Interface | 2D View Controls

See also the Rulers, Guides and Snap Grid section.

Pan

Click and hold the Left mouse button and drag the mouse about to Pan - Esc to cancel mode

Shortcut: Click and drag the Middle mouse button or if using a 2 button mouse, Hold Ctrl + drag with Right Mouse button.

Zoom Interactive

Mouse with Middle Wheel - Scroll wheel in / out

Mouse without Middle Wheel - Hold Shift + Push / Pull with Right Mouse button.

Zoom Box

Click top left corner, hold mouse down and drag to bottom right corner and release. Clicking the left mouse button will zoom in, Shift + click will zoom out.

Zoom Extents

Zooms to show material limits in the 2D window

Zoom Selected

With objects selected

Zooms to the bounding box of the selection

Interface | 3D View Controls

3D Twiddle

Click and drag Left mouse button in the 3D window

Zoom

Right mouse button - Push / Pull

Mouse with Middle Wheel - Rotate wheel

Pan

Click and drag Right mouse button and hold Ctrl.

Click and drag Right and Left mouse button

Click Middle mouse button

Zoom to Fit

Zooms the whole 3D part to fit within the current 3D View window

Isometric View

Shows the model in a 3D isometric view in the 3D window

Plan View (Down Z)

Shows the top view of the model in the 3D View looking down the Z axis.

Press Shift to show the bottom.

Side View (Along X)

Shows the side view of the model in the 3D View looking along the X axis.

Press Shift to show the opposite side.

Side View (Along Y)

Shows the side view of the model in the 3D View looking along the Y axis.

Press Shift to show the opposite side.

Rotate around model (Rotary)

Rotate clockwise / anti-clockwise around the model (Available only in a Rotary project with Wrapped View

Interface | Calculation Edit Boxes

Numerical edit boxes generally support simple calculations.
A sum can be entered directly into the edit box:

Having typed an equation, pressing the = key will perform the entered calculation and fill the edit box with the answer.

Special Calculation Characters

As well as the simple numerical calculations, such as 3+(4/5), several of Cut2D Pro's stored values can be accessed by using certain letters (which are not case-sensitive): When used, Cut2D Pro substitutes the character with the appropriate value in the calculation.

Character

Name

Example

Description

W or X

Material Width

w/2=

Half of the material width

H or Y

Material Height

H*2=

Twice the height of the material

T or Z

Material Thickness

t-0.25=

0.25 units less than the material thickness

P

PI (3.141593)

P*10^2=

Area of a 10 radius circle (π.r2)

I

Imperial Conversion

25.4*i=

Converts 25.4mm to inches

M

Metric Conversion

2*M=

Converts 2 inches to millimetres

'

Feet

2'+10=

34 inches (2 feet and 10 inches)

Interface | Document Variables

Document Variables provide a mechanism for defining values that can be used in Cut2D Pro's Document Variables. They can either be created in the Document Variables dialog which is accessible under the Edit menu, or created from any Calculation Edit Box which supports variables by right clicking and selecting Insert New Document Variable from the Popup Menu.

Naming Document Variables

New Document Variable names must begin with a letter and then may consist of letter, number and underscore characters. Once created, they may be edited in the table beneath the New Variable section of the Document Variables Dialog.

Variables can be exported to a text file and imported into another job. When importing, any existing variable values with the same name will be replaced.

Deleting Document Variables

Variables may be deleted if they're not being used in any toolpath calculations but only when there are no toolpath creation forms open.

Using Document Variables

Once created a Document Variable may be used in any Calculation Edit Box by enclosing its name within a pair of curly braces as illustrated in the figure below.

Right clicking in a Calculation Edit Box provides a Popup Menu that provides shortcuts for creating new Variables and inserting existing variables into the Edit Box.

Once a Document Variable has been created from the Popup Menu it will be inserted into the Edit Box.

Accessing Document Variables

Declared Document Variables can be easily accessed from a calculation edit box. Right-click on the calculation edit box and you will be presented with a menu showing the document variables available currently, as well as an option to quickly insert a new document variable.

Interface | File Types

CRV3D

Files previously created and saved in Cut2D Pro will be opened and displayed in the 2D Design window and 3D View if they contain 3D data. All calculated toolpaths are stored/opened from the CRV3D file.

CRV

Files previously created and saved in Cut2D Pro will be opened and displayed in the 2D Design window. All calculated toolpaths are stored/opened from the CRV file.

DXF
DWG

Files from other CAD or graphics software packages such as AutoCAD will be opened in the original size and position. The Job Setup Form is automatically opened showing the maximum X and Y dimensions of the opened design. The actual size of the material can then be specified along with the required thickness and appropriate X0, Y0 and Z0 origins.

EPS

Files from typical design software such as Corel Draw can be opened. The Job Setup form will automatically be opened so the required material size can be specified. By default the EPS file will be placed with the lower left corner of the design at X0, Y0.

AI

Files from typical design software such as Adobe Illustrator and Corel Draw can be opened. The Job Setup form will automatically be opened so the required material size can be specified. The AI file will be placed with the lower left corner of the design at X0, Y0

PDF

Software such as the Adobe product range can be used to convert files from other design and word processing software into the industry standard PDF file format. The text and vector content of PDF files is extracted when imported into Cut2D Pro. When importing multiple page PDF documents each page is placed on a separate layer.

SKP

SketchUp files with a .SKP extension (see www.sketchup.com) can be imported as 2D data suitable for machining.
See the Sketchup section for detailed instructions on importing Sketchup files.

Interface | Job Setup - Double Sided

The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.

In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.

Job Type

Single Sided job type should be used when design only requires the material to be cut from one side. This is the simplest type of job to design and machine.

Double Sided Job type is useful when it is desired to cut both sides of your material. Aspire allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file.

Rotary job type enables the use of a rotary axis (also called a 4th axis or indexer).Aspire will provide alternative visualisation, simulation and tools appropriate for rotary designs.

Job Size

This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).

It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).

Z Zero Position

Indicates whether the tip of the tool is set off the surface of the material (as shown in the diagram) or off the bed / table of the machine for Z = 0.0.

Zero off same side

This option allows Z Zero to reference the same physical location, regardless whether material is flipped or not

XY Datum Position

This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's posi

Use Offset

This option allows the datum position to be set to a value other than X0, Y0.

Flip Direction Between Sides

This section gives choice between horizontal and vertical flipping when changing machining side. Aspire uses that information to correctly manage the alignment of the geometry relating to each side.

Design Scaling

When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click .

Modeling Resolution

This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.

As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.

The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.

As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.

Interface | Job Setup - Rotary

The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.

In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.

Job Size

Length

Length of the material

Diameter

Diameter of the material

Units

Whether the job units are measured in mm or inches

Z Zero Position

Indicates whether the tip of the tool is set off the rotation axis (as shown in the diagram) or off the surface of material for Z = 0.0. For the best accuracy using Cylinder Axis option is recommended

XY Datum Position

This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's posi

Use Offset

This option allows the datum position to be set to a value other than X0, Y0.

Orientation

This option selects along which axis the material block will rotate.

  • Selecting Along X Axis means that X coordinates represent movement along the cylinder, whereas Y coordinates represent the angle around the cylinder.
  • Selecting Along Y Axis means that Y coordinates represent movement along the cylinder, whereas X coordinates represent the angle around the cylinder.

Flip Design

When this option is enabled, the design will be flipped when the orientation is changed

Design Scaling

When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click .

Modeling Resolution

This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.

As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.

The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.

As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.

Interface | Job Setup - Single Sided

The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.

In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.

Job Type

Single Sided job type should be used when design only requires the material to be cut from one side. This is the simplest type of job to design and machine.

Double Sided Job type is useful when it is desired to cut both sides of your material. Aspire allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file.

Rotary job type enables the use of a rotary axis (also called a 4th axis or indexer).Aspire will provide alternative visualisation, simulation and tools appropriate for rotary designs.

Job Size

This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).

It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).

Z-Zero Position

Indicates whether the tip of the tool is set off the surface of the material (as shown in the diagram) or off the bed / table of the machine for Z = 0.0.

XY Datum Position

This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's posi

Use Offset

This option allows the datum position to be set to a value other than X0, Y0.

Design Scaling

When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click .

Modeling Resolution

This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.

As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.

The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.

As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.

Interface | Job Setup Form

The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited. It allows to create following types of job:

Interface | License Dialog

The License Dialog is used to set the details you need to activate the software. This dialog can also be used to activate optional modules. The page that initially appears will give you the option to set your license details either automatically from your V&Co account or manually.

The "Online Method" section below covers the process to follow if Online is selected.

The "Manual Method" section below shows the process to follow if you wish to type in your license details manually or do not have an Internet connection available.

Online Method

This method will allow you to retrieve your details automatically from your V&Co account. To use this select 'Online' and then click on the form. The online section of the form will then be displayed.

[object Object]

Pressing on this dialog will launch a web browser which will take you to the V&Co login page if authentication is required.

[object Object]

After logging in here with your V&Co account details another page may appear asking for permission for Cut2D Pro to access your license details.

This page will only appear if you have not already granted access. If this appears you should select "Allow" to enable Cut2D Pro to retrieve your license details automatically.

[object Object]

At this point Cut2D Proshould be being displayed and the dialog should be automatically populated with any licenses available on your account.

[object Object]

You can select any of the product licenses available and information on the type of license will be displayed in the status area. Once the license and any modules have been selected by clicking on them can be pressed to activate these and proceed to the summary page.

Note

If there is only a single license available on your account the above page is skipped and the summary page (below) will already be displayed.

[object Object]

This page displays the selected license and module details. If you are changing current license details or adding a module a restart will be required for these to fully take effect. In this case a check box will appear allowing you to restart automatically. If this is checked then when you press Cut2D Pro will automatically be restarted to apply the license changes. If you do not select this option the license changes take effect the next time Cut2D Pro is restarted.

Manual Method

The manual method allows entry of license details without requiring an Internet connection. Selecting "Manual" and clicking will cause the manual entry form to be displayed.

[object Object]

The "Registered User Name" from your license information should be entered into the "Licensed To" area of the form and the license code can either be copied and pasted into the middle row of the dialog or manually typed into the lower section if "Enter license code manually" is selected. The button will become available when a code of the expected length has been entered.

If the product is already licensed then a module code can be entered at this stage instead of the product code. If you wish to manually activate both a product and module code the product code should be added here and there will be an opportunity to add the module code later. Pressing will set the license and display the summary screen.

[object Object]

The summary screen shows the current licensed user and has an button to allow additional modules to be added. Pressing this button will display the manual entry form again and allow the module details to be entered.

If the licensed user is changed or a new module is added a restart will be required for these to take full effect. In this case a check box will appear allowing you to restart automatically. If this is checked then when you press the finish button the program will automatically be restarted to apply the license changes. If you do not select this option the license changes take effect the next time the program is restarted.

Interface | Options Dialog

Note

Many of the choices in this dialog will not take effect until the software has been exited and restarted.

Window Layout

Save Tab Layout

Save the layout and the 'pinned' state of the command and toolpath fly out tabs.

Save Dialog Layout

Save the size, position and visibility for dialogs such as the Layer control and Toolpath Control dialogs.

Save View Layout

Save the layout of the 2D and 3D view windows.

Display Splash Screen

Display the program Splash Screen, while the program is loading.

Top Side Ruler Color

The colour of the ruler on the top side in a two-sided project.

Bottom Side Ruler Color

The colour of the ruler on the bottom side in a two-sided project.

3D View Settings

Shaded Background Style

Allows to choose between Solid, Gradient and Image background styles.

Background Color

Change the background color used for the 3D view. Used with Solid and Gradient background styles.

Gradient Background Color

Change the bottom (lightest) color used for the 3D view. Used with Gradient background style.

Draw Origin

Draw the origin arrows by default on startup.

Draw Material Block

Draws Material Block boundaries by default on startup.

Use Color Shaded View

Draw shaded model in 3D view by default on startup.

Print 3D View Shaded Background

Include the shaded background when printing.

Animate Camera Moves

Switch on/off animation in the 3D View when selecting View positon from the Iso View, Down X, Down Y or Down Z icons.

Image File Path

Path to the image to be used as background. Used with Image background style.

Toolpath Settings

Show Toolpath Operations with Preview

When the toolpath Preview form is visible, keep the 'Toolpath Operations' section visible (requires more screen space).

Auto Open 3D view

Automatically swap to 3D view after calculating a toolpath.

2D Solid Preview Color

Color used to draw the solid 2D toolpath preview with.

Create 2D Previews

Create 2D previews of toolpaths in 2D view.

Select Sheet When Edit Toolpaths

If a toolpath is associated with a sheet, select sheet when edit toolpath.

Toolpath Geometry Fixing Timeout

Number of seconds the program will spend trying to fix problems with geometry when calculating toolpaths.

Drop Tool

When projecting a toolpath onto the model, drop the tool on surface rather than project. If this is set, the toolpath will follow the surface of the model better, but could be slower to calculate.

2D Toolpath Tolerance

Tolerance to apply to 2D toolpaths after calculating to reduce file size.

3D Toolpath Tolerance

Tolerance to apply to 3D toolpaths after calculating to reduce file size.

VCarve Toolpath Tolerance

Tolerance to apply to VCarve toolpaths after calculating to reduce file size.

Note

We strongly recommend that the Toolpath Tolerance should be left at their default settings unless different values are recommended by your machine tool manufacturer. If you do have a machine which struggles with the default settings, try doubling the values and cutting a test-piece to assess the tradeoff between machining times, file size and final machined quality. We have done some limited testing and on a sample complex 3D model, increasing the '3D Toolpath Tolerance' to 0.001 inches gave a 40% decrease in file size and no noticeable difference in quality on the test machine and job. In the test case there was no measurable difference in machining time on the CNC machine the test was carried out on.

Maximum Toolpath Undo Stack Size (MB)

Maximum size in MB of Toolpath data undo stack for storing toolpath delete state.

Append duplicated toolpath

When duplicating a toolpath, this determines whether it places the new toolpath next to the original or append it to the end of the list.

Use new raster

Generate raster toolpaths that are more consistent in regards to machining direction, even for complex shapes.

V-Carve Vector Intersection Check

This option determines whether or not to check for vector intersections when calculating a V-Carve toolpath and what to do when they are detected.

General Settings

Use Graphics tablet

Switch on support for graphics tablet drivers, if installed - for use with the sculpting tool.

Process User Files

Enable/disable processing of files in the 'Vectric Files' folder in your common user document folder.

Recent File List Size

This sets the maximum number of items that will be displayed in the Recently opened files... list in left hand side bar of the interface when there is no file currently loaded. The list will not increase in size until the software has been re-started and more files have been opened and/or saved.

Show the clipart Subfolder Contents

If set to Yes then this will show the contents within the selected Folder in the Clip Art browser along with up to 3 sub-folders if they exist and contain appropriate file types. If set to No it will only display the contents of the selected folder, not sub-folders.

Always open local documentation

Force open the local copy of the documentation when accessed through the Help menu. Cut2D Pro automatically opens the local documentation if you have no internet connection or if the server is taking too long to respond.

Smooth Join Vectors

Produce a smoother join between 2 vectors. This is option is there mainly to support older behavior.

Default to last used text anchor position

Control the default location of the anchor when creating a text object. This is to either default it to the last set location, or always default to a specific location.

File Dialog Default

This option controls the default directory that is opened when opening or saving files. The default Global options will open the last used folder as per the Operating Systems default behavior. If you choose Operation, the software will remember the last used folder for that particular operation. We divide operations in broad categories, such as, vector import / export, model import / export, toolpaths, tools, etc... If you choose Job, we will always default to your saved job's location.

Interface | PDF Export

The PDF Export form allows vectors within your drawings to be exported into PDF format.

Vector(s)

Export All

Selecting this option will export all of the vectors contained on the specified sheets and layers.

Export Selected Only

Selecting this option will export only the vectors which are currently selected and on the specified sheets and layers.

Sheets

The sheets you wish to be exported to PDF can be selected from within this section. Clicking will deselect all of the sheets and clicking will cause all of the sheets to become selected. You can also manually select/deselect individual sheets by clicking on the check box to the left of the sheet name.

Note

Each sheet will be saved as a separate page within the PDF file.

Layers

The layers you wish to be exported to PDF can be selected from within this section. All the visible layers with content on them will show up in this list.

When All visible layers is chosen all of the vector layers will be selected. Only vectors on the layers selected will be exported into the PDF file. When Selected layers only is chosen individual layers can be manually selected/deselected by clicking on the check box to the left of the layer name.

Options

Export Job Bounds - If this option is selected a vector representing the boundary of the job will also be output to the PDF file.

Clicking will prompt you to choose a filename and location for your file and save your drawing in PDF format at that location.

Interface | SketchUp Files

SketchUp files with a .SKP extension (see www.sketchup.com) can be imported as 2D data suitable for machining into a Cut2D Pro job using the File ► Import Vectors... command from the menu bar or the import vectors icon on the Drawing tab. To import data from a SketchUp file you must already have created or opened a job to import the data into.

As a SketchUp model is usually a 3D representation of the part, the SketchUp importer offers a number of options to allow you to start manufacturing the model.

We will illustrate the two main choices for how the model will be imported using the SketchUp model shown to the left.

The model shown in the screenshots is a cabinet constructed by following the instructions in the Fine Woodworking 'Google SketchUp guide for Woodworkers: The Basics' DVD which is available via the Fine Woodworking site at www.finewoodworking.com. Vectric have no affiliation with Fine Woodworking, we are just using screenshots of the model constructed while following their tutorials to illustrate the process of importing a SketchUp model.

Layout of Imported Data

In the first section there are two main choices for how the data from the model will be imported, 'Exploded Flat Layout' and 'Three Views - Front, Top, Side' as shown below.

Exploded Flat Layout
Exploded Flat Layout
Three Views - Front, Top, Side
Three Views - Front, Top, Side

Exploded Flat Layout

This option will take each component in the model and orientate it flat ready for machining.

Once this option is selected a number of sub-options also become available.

Part Orientation

This section controls what Cut2D Pro considers to be the 'top' face of each part.

Auto Orientate

If this option is selected, for each part in the model, the 'face' with the largest area based on its outer perimeter (i.e. ignoring holes etc.) is considered to be the 'top' face and the part is automatically rotated so that this face is facing upwards in Z. This strategy works very well for models which are to be manufactured from sheet goods where there are no features on particular faces which need to be on the 'top' (such as pockets).

Orientate by material

This option allows the user to control more explicitly the orientation of each part in the model. Within SketchUp the user can 'paint' the face of each component/group with a material/color of their choice to indicate which face will be orientated on top when the model is imported. When this option is selected simply chose the material which has been used to indicate the top face from the drop down list. If a part is found in the model which does not have a face with the specified material, that part will be oriented by making the largest face the top.

Gap between parts

This field lets the user specify the gap between parts when they are first imported. After importing, the nesting functions within Cut2D Pro can be used to layout the parts with more control and across multiple sheets.

Three Views - Front, Top, Side

This option will create an 'engineering drawing' style layout of the SketchUp model as shown in the screenshot below.

The size of the model is preserved and it is relatively simple to pick up dimensions for parts you are going to manufacture from the various views. The colors of the lines you see are taken from the colors of the original SketchUp layers the various parts of the model are on.

Create Circles / Arcs

SketchUp does not maintain true arc or circle information for the boundaries of its parts. This is a problem when it comes to machining as the 'polygonal' SketchUp representation can give very poor machining results. For this reason, Cut2D Pro offers the option to refit circles and arcs to imported data.

Options Checked ✓
Options Checked ✓
Options Unchecked
Options Unchecked

The screenshot above left shows the results of importing a part with a filleted corner and hole with these options unchecked. The 'fillet' is made up of a series of straight line segments and the circular 'hole' is actually a polygon made up of straight lines.

The screen shot above right shows the same part imported with both these options checked ✓. The 'fillet' now consists of a single smooth arc and the circular 'hole' now also consists of arcs rather than straight line segments. Both these features will machine more cleanly in this form.

Data to Import

A SketchUp model will often contain parts that you do not wish to machine (such as hinges, knobs etc.) or data which will be cut from different thicknesses of material and hence different parts need to be imported into different Cut2D Pro jobs. To allow control over what is imported you can choose to only import parts of the model which are on particular layers using this section of the dialog.

To only import data from selected layers, choose the 'import visible data on selected layers' option and click the check box next to each layer to indicate if you want to import data from that layer. Note that the number of parts on each layer is displayed next to the layer name.

It is very easy to assign different parts of the model to different layers within SketchUp to help with the import process into Cut2D Pro. The screenshot below shows the result of only importing data on the 'Door' layer from the example.

Component / Group Handling

This section of the form allows advanced handling of how 'parts' within the SketchUp model are identified and treated on import.

Group imported parts

This option is normally selected for all but the simplest models as it allows each 'part' of the model to be selected, moved and nested easily after import. You will need to ungroup the imported data after nesting etc. to allow individual features to be machined. By default, Cut2D Pro will treat each SketchUp group / component as a single part UNLESS it contains other groups or components within it, in which case each lowest level group / component will be treated as a separate part.

Items which you retain in groups can be ungrouped at any time in the usual ways.
If the right-click menu-option to Ungroup back onto original object layers is used (which is the default option when using the icon or shortcut U) then the software will place the ungrouped items back onto the original layers they were created on in SketchUp.

Keep components starting with two underscores (__) together

If you have a complex model which contain 'parts' which are made up of other groups / components, you will need to do some work on your model to identify these parts for Cut2D Pro. The way this is done is by setting the name of the groups / components that you wish to be treated as a single part to start with__ (two underscore characters). For example, if you had a model of a car and you wanted the wheels / tires / hub nuts to be treated as a single part even though the Tire, Wheel and other parts were separate components, you would group the parts together and name them something like __WheelAssembly in SketchUp. When this model was imported, and Cut2D Pro reached the group/component with a name starting with __ it would treat all subsequent child objects of that object as being the same part.

Replace outer boundary (for flat jobs only!)

There is a style of 'building' with SketchUp where individual 'parts' are made up of several components 'butted' against each other. The screenshot below shows such a component.

This object is made up of many smaller components representing the tabs on the top, the connectors at the end and the support at the bottom as shown below.

Although when can treat this as a single 'part' when imported by starting its name with __ (two underscores), the imported part is still going to be difficult to machine. The screenshot below shows the part imported into Cut2D Pro without the 'Replace outer boundary' option checked ✓. The part in the image has been ungrouped and the central vector selected.

As you can see, the outer boundary is made up of separate segments for each 'feature'. Cut2D Pro does have the ability to create an outer boundary for vectors but this can be time consuming if it has to be done manually. If the 'Replace outer boundary' option is checked, ✓ for every part Cut2D Pro will try to create a single outer boundary and delete all the vectors which were part of this boundary. The screenshot below shows the result of importing the same data with this option checked, ✓ this time the part has been ungrouped and the outer vector selected.

This data is now ready to be machined directly. It is important to understand the limitations of this option. It can be substantially slower. Creating robust boundaries for each part can consume a lot of processing power. Any feature which shares an edge with the boundary will be deleted. If the tabs on the top of this part were to have been machined 'thinner', this approach would not have been suitable as the bottom edge of the tabs has been removed.

IMPORTANT

The new features will help a lot of SketchUp users dramatically reduce the time it takes to go from a SketchUp design to a machinable part using Vectric Software. It is important to understand though that while these options provide a useful set of tools, in many cases there will still be additional editing required to ensure the part is ready to toolpath. Understanding the options and how they work will allow the part to be designed in SketchUp with these in mind and therefore help to minimize the time to machine once the data is imported.

Note

Sketchup files will only open in the same bit version you are running e.g. A file saved in a 32 bit version of Sketchup will only open up in a 32 bit version of the software.

Interface | View Controls

Your project is represented using 2D and 3D workspaces, each viewed via independent windows; the 2D View and 3D View, respectively. This division usefully maps to the typical workflow in which you will initially focus on the 2D design and layout of your project before moving to the 3D stage of modeling, toolpathing and previewing your finished part.

You can switch between the views using the tabs at the top of each window. In addition the shortcut-keys F2 and F3 will toggle the display between the two windows.

It is sometimes useful to see both the 2D and 3D representations at the same time. The Page Up and Page Down keys will arrange the 2 views either horizontally or vertically so you can see both workspaces simultaneously. To return to the tabbed display, simply click on the standard Windows Maximize button in the top right corner of either view window.

Many of the controls for manipulating the view in your project are similar in both 2D and 3D.

From within each view you can also directly interact with the objects that make up your job using the Object Selection Tools.

Interface | View Toolbar

[object Object]

Above the view window is a handy toolbar that allows easier access to common tools. With the ability to create a double sided project you have easy access to switch between the Top and Bottom Sides of your project. The Layers Drop down bar has now moved from the drawing tab to the View Toolbar, making it accessible at all times. The other icons displayed in order of left to right are as follows

Snapping Toggle Options

Snap to geometry

Smart Snapping

Snap to Grid

View Controls

Toggle Pan / Twiddle View

Zoom to box

Zoom to drawing

Zoom to selection

Toolpath Drawing Toggle

Toggle 2D Toolpath Drawing

Toggle solid 2D Toolpath Drawing

3D Drawing

Toggle drawing of material block

Tile 2D & 3D View Windows

Stack 2D and 3D View windows vertically

Stack 2D and 3D View windows horizontally

Two-Sided Machining

When you are working on a two-sided job additional icons will appear on the View Toolbar. On the left you will see an icon indicating whether the job you are working on will be flipped horizontally or vertically. This is important because the software will automatically mirror your toolpaths and geometry around different axes depending on this setting. To maintain the correct alignment of your toolpaths you must physically turn the material on your CNC machine in the same direction as you have specified during the design process.

Turn horizontally from left to right

Turn vertically, end over end

Note

This icon is just for you information and does not perform any operation; it is not clickable.

The next button indicates which side you are currently working on. It is a toggle button that can be clicked. Clicking this button swaps the active side of your job.

Top side is active, all operations will apply to the Top side.

Bottom side is active, all operations will apply to the Bottom side.

Note

The rulers that border the 2D View are colored to provide a handy visual indicator as to which side is currently active. An Orange background indicates that the Bottom side is currently active and any drawing or toolpaths are associated with the Bottom Side of your design.

The final additional tool for two-sided job is on the right hand side of the View Toolbar and it allows you to toggle the 3D composite relief to show either the currently active side or your model only, or both sides of your model as a single solid block.

Toggle Two-Sided View

Menus | Edit

Undo

Steps backwards through the last 5 changes made by the user.

Redo

Steps forward through design steps that have been Undone using the Undo command (see above) to get back to stage that the user started using the Undo function.

Cut

Removes the selected objects from the job and places them onto the clipboard.

Copy

Copies selected objects to the clipboard, leaving the original in place

Paste

Pastes the contents of the Clipboard into the model (see cut and copy above).

Delete

Deletes the selected object - same as hitting the Delete key on your keyboard

Selection►

Select various types of vectors

Align Selected Objects ►

Give the user all the options covered under the Align Objects section of the menu.

Opens the Alignment Tools form.

Join Vectors

Joins open vectors.

Opens the Join Vectors form.

Curve Fit Vectors

Allows arcs, Bezier curves or lines to be fitted to existing vectors to 'smooth' them.

Opens the Fit Curves to Vectors form.

Nest Selected Vectors

Opens the Nesting form.

Job Size and Position

Opens the Job Setup form.

Notes

Opens a text box where you can record notes regarding this job, such as customer name, material required, special setup instructions or any other relevant text information you would like to keep when you save the job.

If the text starts with a period/full stop/dot '.' , the Notes dialog will be displayed automatically each time the file is opened. The text from the Notes dialog can also be optionally output into the toolpath as a comment field. See the Post-Processor Editing Guide.

Document Variables

Opens the Document Variables dialog.

Snap Options

Opens the Snap Options dialog.

Options

Opens the Program Options dialog to allow the customization of certain aspects of the program.

Selection

Select All Vectors

Selects all the currently visible vectors in the part (vectors on invisible layers are not selected).

Select All Open Vectors

Selects all the currently visible Open vectors in the part

Select All Duplicate Vectors

Selects all the currently visible Duplicate vectors in the part - these are vectors which are exact copies of each other in terms of shape and location so that visually they appear to be only one vector. These can cause problems for some toolpath and modeling functions so it can be useful to delete them or move them to a new layer.

Select All Vectors On Current Layer

Selects all the vectors on the selected layer.

Unselect All

Deselects all the currently selected vectors in the part

Vector Selector...

Opens the Vector Selector dialog.

Menus | File

New

Creates a New Cut2D Pro job.

Open...

Opens an existing Cut2D Pro job

Close

Closes the current file but leaves the software running

Save

Saves the current Cut2D Pro file over the last saved version of the file.

Note

This command will overwrite the old file with any changes made since the last save. If you are not sure of your changes then use the File ⇒ Save As... command instead option and give the file a new name.

Save As...

Opens the standard File Save dialog so you can save the current file with a new name.

Increment and Save

The Increment and save operation allows you to automatically number iterations of files you are working on. If you select this operation when editing a file which ends with an underscore, or a hyphen followed by a number, then the number will be increased by 1 and the file will be saved using this number.

For example, MyFile_1.crv3d becomes MyFIle_2.crv3d MyFile-1.crv3d becomes MyFile-2.crv3d

Note

The increment and save option will keep incrementing until it finds a file that does not currently exist. It will not overwrite an existing file.

Print

Opens the Print Setup box to Print your design

Print Preview

Displays a Preview of the design to print

Print Setup

Opens the Print Setup box to Print your design

Import... ►

Import various entities into the job

Export... ►

Export vectors from the job

Open Application Data Folder...

Opens the Windows folder where files used by the software are stored. This is useful for adding to the default files installed initially.

Application files include: Bitmap textures for creating custom materials. Gadget scripts for customized automation of the software. Postprocessors The Tool Database Default toolpath strategy settings Vector texture files.

Exit

Closes the job and exits the software.

Import

Import Vectors...

Import Vector data.

Import Bitmaps...

Import Bitmap data

Import Component / 3D Model...

Import 3D Model or Component

Import PhotoVCarve or Cut3D Toolpaths...

Import a toolpath file created in another Vectric application, such as, Cut3D or PhotoVCarve.

Export

Allows you to export selected Vectors as either an eps, dxf, ai, svg or pdf format vector file. If no vectors are selected, the all visible vectors will be exported.

Note

When exporting in DXF format, the layer information relating to the exported vectors is preserved.

Printing and Print Preview

The contents of either the 2D or 3D view can be printed using the Print... command on the File menu. Simply select the view you wish to print (2D or 3D) and then click the Print... command. The standard Windows printer dialog allows you to select the printer and adjust its properties. When the OK button in this dialog is clicked, the view will be printed. To adjust the printer settings without printing, you can open the same dialog using the Print Setup... command on the File menu. When used in this way, the button on the dialog will store the settings without printing immediately.

Note

By default printing the 3D view does not print the shaded background; this behaviour can be changed using the Options dialog, which is opened using the Options command on the Edit menu.

The Print Preview... command on the File menu allows you to check the layout of your page before you print. If you are happy with the preview, use the button to begin printing the document directly from the Print Preview page.

Note

The printed view is always scaled to exactly fit the currently selected page size (including allowance for margins). Drawings are not, therefore, printed at actual size and are not printed across multiple pages.

Menus | Gadgets

Gadgets are small programs that add additional functionality to Cut2D Pro, VCarve Pro and Aspire. They can be used to add new features to the software or automate common sequences of tasks. Examples include adding the ability to cut dovetail style joints with a standard end mill and applying toolpath templates to every sheet in a nested job followed by automatically post-processing and saving the files for your machine tool.

Install New Gadget...

Opens a standard Open File Dialog that allows you to chose a downloaded gadget you want to install.

Gadget Shortcuts

Opens Gadget Shortcuts dialog.

Installing Gadgets

You can expand your Gadgets library by downloading and installing more from the Gadgets website.

These Gadgets will install into your public documents folder (Public Documents/Vectric/Cut2D Pro/Gadgets). If you wish to delete any of these Gadgets, simply navigate to the location above and delete the folder.

Each Gadget has specific requirements in order for it to run, it is recommended that you read the instructions in full before use. Some Gadgets require that you select vectors before running the Gadget, others may need to be run before a job in the software is created. When there is a requirement that has not been met before running, you will receive an error message, stating which requirement has not been met.

Note

It is important to point out that the gadgets are NOT as polished as functionality which has been integrated into the main program. The gadget concept is intended to allow Vectric to produce simple add-ons which address minority requirements without cluttering up the main interface. As the Gadget library grows over time, we do not expect users to install every gadget, but only those that may be relevant to tasks they actually perform.

Running Gadgets

Installed Gadgets are accessible from the main Gadget menu, which is built dynamically each time Cut2D Pro starts up.

Alternatively Gagdets can be assigned shortcuts.

Gadget Shortcuts

Shortcut can be set to run a chosen gadget from the list of gadgets. To set the gadget shortcuts select the Gadget Shortcuts button from the Gadgets menu.

You may then assign one of the predefined shortcut keys to run a chosen gadget. The available shortcut keys are Ctrl and a function key.

Preinstalled Gadgets

A number of Gadgets are included as part of the default installation of Cut2D Pro. These are all available from the Gadgets menu:

Wrapping Sub-menu:

Note

We ship some gadgets which help perform common tasks for people with rotary axis. If a user has no interest in rotary machining, they can delete the 'wrapping' gadgets from their gadgets folder and those options will no longer be available from the Gadgets menu.

Developing Gadgets

Gadgets can also be created by our users using the LUA scripting language, we provide an SDK and tutorials on the gadgets website.

Please Note

This will require knowledge of programming.

The SDK and the Tutorials are provided as is, Vectric cannot provide support on the development of user Gadgets.

Gadgets have their own section on the Vectric Forum, you can get news on the latest releases from Vectric and fellow users.

Menus | Help

Help Contents

Displays an online version of the full reference manual that documents every feature and option available in the software.

Note

The reference manual is not intended as a User Guide or introductory training resource - please don't forget about the Getting Started guides and the extensive video tutorial library on your install media.

Keyboard Shorcuts

Displays the Shortcut Keys

Video Tutorial Browser...

Access the tutorials

What's New

See a summary of the new features added in major and minor updates.

Release Notes

See the list of issues fixed and enhancements in patch updates.

Third Party Licences

Display a list of all the third party software used to help create Cut2D Pro.

Enter License Code

Displays the License Dialog used for entering license or module details.

View the Vectric Online FAQ...

Displays the Frequently Asked Questions (FAQs)

View the Vectric User Forum...

Opens the Vectric User Forum in your Web Browser if you have an Internet Connection. Everyone should join the Forum to engage with other users and benefit from each others tricks and tips!

Visit Vectric Support online...

Opens the Vectric Support Website in your Web Browser if you have an Internet Connection.

Visit Vectric User Portal...

Opens the Vectric User Portal in your Web Browser if you have an Internet Connection. Download software installation files, activation codes and Clip Art included with the software.

Post Processor Editing Guide

Opens the page explaining how to create and edit your own post processors.

Migrate From Older Version

Opens a dialog to enable the settings in the last version of Cut2D Pro to be copied to the latest version.

Check for Updates

Try this periodically to check (through the Internet) if an update is available for your software.

About Cut2D Pro...

This window displays the version of the software being used, to whom the software is license and the type of license.

Menus | Model

Create Component ►

Create Component From... ►

Create Component from Bitmap

Import Component / 3D Model

Export as STL

Export as Grayscale Bitmap

Export as 3D Clipart: Exports the selected model as a .3DClip file.

Sculpt Visible Model

Smooth Selected Components

Reset Inside Selected Vectors: Deletes everything in the Working Model contained inside the selected vector(s)

Reset Outside Selected Vectors: Deletes everything in the Working Model contained outside the selected vector(s)

Split Selected Component: Split the currently selected component using a vector.

Create Vector Boundary Around Selected Components: Creates a new vector that matches the edge of the selected component.

Emboss Component

Scale Model Z Height

Distort Selected Component

Replace Below

Selected Component Properties

Create Component

Create Shape From Vectors

Two Rail Sweep

Extrude and Weave

Turn and Spin

Create Textured Area Component

Add Zero Plane: Creates a component that is the size of your job setup with a height of Zero.

Create Component From...

Export As Grayscale Bitmap

This is export option will save the Composite Model (Working Model + visible Components) as a raster based image file (.bmp/.jpg/.gif format). This is mainly intended for users of Laser engraving equipment and CarveWright/CompuCarve machines. It could also be used to export the 3D as a grayscale for use with graphics programs.

When the image is exported the highest areas in the model will be white and the lowest will be black, all the other depths in between will be assigned graduated levels of gray depending on their relative position between the top and bottom of the part.

Composite Model
Composite Model
Saved Grayscale image
Saved Grayscale image

To use this function you must have either visible Components or something in the Working Model.

Create Component from Toolpath Preview

This will take the current Toolpath Preview and create a Component model from it. There are two main applications for this feature:

  • It can be useful for helping to identify areas which have not been machined so a smaller tool can be used to carve them with more detail.
  • It can be used to create model Components where some of the shape has been created using the tool shape such as fluted veins on a leaf or a texture toolpath]. This second application would be particularly beneficial for customers who plan to save a grayscale image of the 3D model (for Laser or CarveWright) rather than running the actual toolpaths from the software.

Once this is selected the current Toolpath Preview will be converted into a Component. This is then added to the Component List and will be called Toolpath Preview.

If the part has been cut-out and the Delete Waste Material option has been used then just the parts left on the screen will become the Component. If the part is not fully cut-out or the waste material has not been deleted then the whole Toolpath Preview block will become the Component, including what may be scrap material. It is possible to avoid this even without deleting the waste by using the Shift key - see below for more information.

By holding down either the Ctrl or Shift key, there are two options that can be activated when the Create Component from Toolpath Preview feature is selected.

If you press the Shift key when you create the Component, the areas of the Toolpath Preview over transparent areas in the composite model will be discarded. This will give you a Component that represents the Toolpath Preview but deletes anything that is not within the area of the 3D model the toolpaths were created on in the first place.

If you press the Ctrl key, the Component created will represent the difference between the composite model and the Toolpath Preview. The model this creates will look odd as it will just represent the material that was left by the radius of the tool on the finish cut. This can be useful if you want to machine those areas with a smaller tool as this model may then be used to create the vectors to limit the toolpath for that operation, minimizing the time to create a more detailed finish.

The images below show the 3 options available. Below left is the standard Component created from a machined model which includes the waste block. The middle option shows the option when the Shift key is pressed which discards the Preview model outside of the original area of the machined part. Finally the right hand image shows the Component which is created when holding the Ctrl key down which is the different between the original part and the Middle image.

Standard Component
Standard Component
Shift Key held
Shift Key held
Ctrl Key held
Ctrl Key held

IMPORTANT NOTE

Although this option can be selected at any time, it only makes sense to use this feature while the Toolpath Preview is active in the 3D View, this will ensure that the Component represents what can actually be seen. The Toolpath Preview can be accessed using the icon in the Toolpath Operations menu (shown below highlighted with a red box), this will also appear automatically after the calculation of any toolpath.

Menus | Right Mouse Click Menus

Clicking the ►RIGHT hand mouse button in different places in Cut2D Pro will display a menu with choices which depend on the area of the software being clicked on and/or the object or selection that the mouse cursor is positioned over. This page details some of these areas and the menus that you will see when RIGHT mouse clicking.

2D View

This menu is displayed when you Right mouse click in 2D View either in the white background of the part or over a selected vector. Most of these options repeat functions and icons described elsewhere in this manual, you should refer to the appropriate section to view how these work.

Layer and Side Operations

The Copy to Layer, Move to Layer, Move to Sheet, Copy to other Side, and Move to other Side options are unique to this Right click menu.

  • Copy to Layer allows you to copy an object onto an existing Layer or to create a New one to copy it onto.
  • Move to Layer gives you the same choices but moves the original object rather than making a copy.
  • Move to Sheet can only be used if you have generated additional Sheets through the Nesting process, in that case it allows you to move objects from one Sheet to a different one from the list available.
  • Copy to Other Side copies the selected objects onto the other side in a two-sided job. It will be transformed so that they match up when looking through the material.
  • Move to Other Side moves the selection similarly to the Copy operation.

Span Editing Menu

If the current selection mode is set to Node Editing, one of two different menus will appear when the user clicks the RIGHT mouse button depending on whether the cursor is currently over a vector Node or a Span of a selected vector in the 2D View. These menus have functions in them that correspond specifically to this selection and position. The menu shown here will appear when the cursor is over a Span of a vector in Node editing mode. You can see a variety of choices: to convert the span to a Line, Bezier (curve) or Arc, Insert a Point, Cut the Vector at that point, Delete the Span, or Insert a Midpoint. Keep Bezier Tangency, which will fix the start and end directions of Bezier curves when they are being dragged directly, can be toggled on or off. From this menu you can also Reverse the direction of the selected vectors, Close any selected open vectors, Join two selected open vectors or Exit node editing mode. Many of these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the keyboard when the mouse is in position (over a node-edit vector span) instead of Right Clicking the mouse button to access the menu.

Node Editing Menu

This menu will appear when the cursor is over a Node of a vector in Node editing mode. You can see a variety of choices: Delete the Point, Smooth it, Insert a point at a virtual midpoint, Cut the vector at that point, change the point to be the Start Point of the vector or extend the vector using the Polyline tool. Horizontal or vertical mirror mode for node editing can be toggled on or off. From this menu you can also close any selected open vectors, Join two selected open vectors, Exit node editing mode or lastly see and edit the exact XY co-ordinate position of the node by selecting Properties. Many of these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the keyboard when the mouse is in position (over a node-edit vector node) instead of Right Clicking the mouse button to access the menu.

Bitmap Properties Dialog

When a Bitmap or Component Grayscale is the selected item in the 2D View and the RIGHT Mouse menu is activated then there will be an additional option in the pop-up menu called Object Properties. This will open the dialog shown below which can be used to fade the Bitmap or Grayscale object strengthen or fade the detail in it when it is not selected. This can be helpful to make it easier to see features perhaps to help you manually trace vectors over it or to fade them so its easier to see vectors that overlap the object.

Toolpath List Menu

When you RIGHT click on a toolpath name within the Toolpath List there are various options you are presented with to alter this toolpath. You can show a toolpath where you have the option to

  • Show This,
  • Show Only This,
  • Show All But This
  • Show All With This Tool
  • Show All.

This toggles the visibility of the Toolpaths according to your choice. The next option allows you to Hide This or Hide All your toolpaths.

You can Edit, Rename or Duplicate the selected toolpath. Selecting Recalculate All will work through the toolpath list recalculating each toolpath with any updated geometry selections.

The last option allows you to delete one or more toolpaths, where you can Delete This, Delete All Invisible, Delete All Visible and Delete All.

Menus | Toolpaths

Show Toolpaths Tab

Can be checked ✓ on or off to pin the Toolpath Tab open or unpin and hide it.

Recalculate All Toolpaths

Recalculate all toolpaths in the project.

Toolpath Drawing ►

Opens the Toolpath Drawing submenu.

Preview Simulation Quality ►

This controls the resolution (number of points) in the Toolpath Preview simulation model governing the amount of detail that the model will display when you Preview and toolpath. The higher the quality, the slower the speed of simulation will become. Guidelines are given on how much slower you should expect it to be but these will depend upon the performance of the PC and relative size of the tool being used to your job (the larger the tool, the slower the performance).

  • Standard is the fastest mode and recommended for low performance PC's.
  • High (2 x Slower) displays better quality images and is for general use.
  • Very High (4 x Slower) displays good quality images, but will run a little slower.
  • Extremely High (8 x Slower) gives good quality images but will run slower on old PC's.
  • Maximum (25 x Slower) gives the best quality image, but could take a lot longer on any PC.

Templates ►

Opens the Toolpath Templates submenu

Merge Visible Toolpaths

Opens the Create Merged Toolpath Form to merge different toolpaths that use the same tool into one optimised toolpath.

Create Job Sheet

Creates a job setup sheet which gives an overview of all of the toolpaths in the job. This opens a File Save As dialog prompting for a place to save the created sheet. The created job setup sheet is a single page of HTML, suitable for viewing in a web browser of your choice, or for printing. This can also be customized with the Job Setup Sheet Editor in the Gadgets Menu.

Install Post Processor

Opens a File Open dialogue box where you can install a post processor.

Tool Database - Material

Opens the Material Management dialog of the Tool Database

Tool Database - Machine Management

Opens the Management dialog of the Tool Database

Tool Database

Opens the Tool Database Dialog.

Toolpath Drawing sub-menu

Draw 2D Previews

Can be checked ✓ on or off to display the toolpath previews in the 2D View.

Make 2D Previews Solid

Can be checked ✓ on or off to switch from the wireframe view to a solid view.

Auto Open 3D View

Selects whether the 3D view and Preview Toolpaths Form are automatically shown after toolpaths are created.

Draw rapid moves

Toggles the visibility of red rapid-speed move lines on the 3D view when toolpaths are visible.

Draw plunge moves

Toggles the visibility of cyan plunge-speed move lines on the 3D view when toolpaths are visible.

Draw retract moves

Toggles the visibility of green retract-speed move lines on the 3D view when toolpaths are visible.

Draw join moves

Toggles the visibility of purple join move lines on the 3D view when toolpaths are visible. A join move is a purely 2D move between toolpath contours, these are typically seen in Offset pattern Pocket Toolpaths.

Templates sub-menu

Save Selected Toolpath as Template

Saves the toolpath that is currently selected as a template for use in another project.

Save All Visible Toolpaths as Template

Saves all of the currently visible toolpaths as a single template for re-use in another project.

Load Template

Loads a previously stored template containing all the settings for one or more toolpath strategies.

Menus | View

Zoom to Drawing

Use when you need to see the whole drawing and material as large as will fit in the 2D View window.

F5

Refresh 2D View

In situations where the complete vector geometry represents a very large job and the user zooms into a small region, the shape of arcs and curves may look faceted. This is only a display issue and will not impact on the quality of toolpaths. This command will rebuilds the display information to correct the graphics being drawn on the screen so curves are drawn smoothly again.

Guide Lines ►

For more details see the section on Rulers, Guidelines and Snapping. Opens the Guide Lines sub-menu.

Draw Origin

XYZ origin arrows can be toggled on and off in the 3D View to show exactly where the X0, Y0 and Z0 origin is position is relative to the material.

Draw Modeling Plane

This option controls the display of the semi-transparent 'modeling plane' which shows the position of the working model base plane.

Draw Material Block

Toggles the drawing of a wireframe representation of the limits of the material block. This is useful for seeing how the 3D model will be positioned in the block of material it is being cut from.

=

Multi Sided View

Allows you to view both sides in the 2D and 3D view when working in a multi sided environment.

Auto-Wrapping View

Allows you to view wrapped toolpaths and models when in rotary job.

Color Shaded View

Draws / Undraws the color shaded job in the 3D window.

Use Shaded Background

Shows either the default gradient filled color background or a solid light blue color background. The solid color is very useful for saving images that need to be cropped out of the background in a graphics software package.

Light follows viewer

The default light setting for the 3D window shines a light onto the job from the top left corner of the material bounding box. Checking ✓ this option can sometimes be used to help visualize the job more easily.

Use Shadow Shading

Toggles the drawing of increased shadows in the 3D view. This can be useful for emphasizing details in models. This degree of shading can be increased or decreased using Ctrl + NumPad+ or Ctrl + NumPad-

Save Shaded Image

Saves a color shaded image of the 3D view as a BMP, JPG, PNG or GIF file.

Note

Saving the image without the color shaded background is often useful when the image will be used on its own in a brochure or on a web site etc. If you select PNG as the file type with the shaded background switched off the image will be saved with a transparent background. To switch the shading off, go to Edit ► Options ► Use Shaded Background and set Use Shaded Background to No.

Page Down

Tile Windows Horizontal

Tiles the 2D and 3D View Horizontally, 2D View at the top and 3D at the bottom.

Page Up

Tile Windows Vertical

Tiles the 2D and 3D View Vertically, 2D View on the left and 3D on the right.

Cascade Windows

Cascades the 2D and 3D View so they overlap.
To Maximise the windows again, double-click the title-bar of either view.

Guide Lines sub-menu

Guides Visible

Toggles the visibility of Guide Lines in the 2D view.

Delete All Guides

Deletes all the Guide Lines in the 2D view.

Lock All Existing Guides

Locks the position of all the Guide Lines in the 2D view.

Unlock All Existing Guides

Allows all the locked Guide Lines in the 2D view to be moved again.

Drawing | Alignment Tools

The Align Objects tool provides a number of options for accurately aligning the selected object to other objects in the selection, or to the available material.

Align to Material

The options in this section will align one or more selected objects within the material workspace defined when you setup your job (the white area in your 2D View).

Center in Material

This option moves the selected items to be positioned in the middle of the material. The short-cut key for this is F9.

Center in Material X only

Align items centrally in the material only moving them along the X axis so the vertical position will not be changed.

Center in Material Y only

Align items centrally in the material only moving them along the Y axis so the horizontal position will not be changed.

Align to Selection

The different items comprising your design in the 2D View can be aligned relative to one another using the following selection sequence:

  • Select the item/s you wish to align / move (use single or multiple selection options).
  • Hold the Shift key down.
  • Select the final item - this is the object that the rest of the selected items will be aligned to Click the required alignment option.

There are 7 alignment options for aligning the selection to the inside edge:

Align Center

Center selected items in the middle (both horizontally and vertically) of the last selected item.

Align Vertical Center

Align the selected items vertically centered to the last selected item.

Align Horizontal Center

Align the selected items horizontally centered to the last selected item.

Align Left/Right

Align the selected items to the left or right edge of the last selected item.

Align Outside Top/Bottom

Align the selected items on the outside top or bottom edge of the last selected item.

Space Selection

The final section is different from the preceding two. The tools here evenly space the selected objects either horizontally or vertically whilst maintaining the relative X or Y positioning of the items. The top and bottom items (for vertical spacing) or left and right items (for horizontal spacing) will remain in place and the other items will be spaced evenly between them.

Alternatively if CTRL is pressed the order of selection will be taken into account and the selected objects will be spaced evenly between the first and last object selected.

If Inside last vector is checked the items will be evenly spaced within the bounds of the last object that was selected.

Show common tools on drawing tab

If this option is checked, ✓ the most common alignment tools will be displayed on the drawing tab in their own section called Align Objects. The Alignment form can still be accessed from the original icon in the 'Transform Objects' section (or by pressing F10).


Drawing | Array Copy

This tool will automatically create copies of the selected object and lay them out in a grid pattern. The grid size is determined from the number of row and columns requested and the spacing of the object copies can be set directly as a gap distance, or in terms of an offset distance between each copy's position.

Selected Objects Size

Reports the current size of the selection that you are intending to block copy. This is for information only, but the values can be selected, copied and pasted to use in other calculations.

Rows and Columns

These options specify how many rows and columns of the selected object to create. The total number of copies made will be X multiplied by Y.

Spacing...

There are two ways to specify the spacing between elements in array:

  • Gap : The X and Y fields will be used to specify the gap between edges of each object copy.
  • Offset : The X and Y fields are used to define the offset of the position of each object copy, relative to the preceding one.

Symmetry...

The symmetry area of the form gives you the ability to mirror and rotate objects. This allows for more advanced pattern making, by default the block symmetry form is set so there is no symmetry or rotation. To alter the pattern you can simply press the block symmetry buttons to create your desired pattern.

[object Object]
Reversing direction of top row

Row/Column displacement...

Entering values in the Row/Column displacement allows you to offset every other row or column by the value specified.

[object Object]
Displacement in x

Group Copies

Having this option checked ✓ will group the objects that you have created in the form when you hit the button.

Drawing | Auto Layout Text

This option automatically sizes a block of text to fit inside the boundary box (width and height limits) of a selected vector or vectors. If no vectors are selected the text is scaled to fit the size of the material.

Entering Text

The procedure for Drawing Text in the 2D Window is:

  • Select the vector inside which the text is to be fitted
  • Click the Draw Text icon
  • Enter the required text content
  • Select the font either True Type or Single Line as required and alignment options

The button opens a larger text entry window that makes it easier to enter text that needs to run on longer line lengths.

Font Selection

Vertical Fonts

Fonts that start with the @ character are drawn vertically downwards and are always left justified

Engraving Fonts

The Single Line Radio Button changes the Fonts list to show a selection of fonts that are very quick to engrave.

This example shows text (in an Engraving Font) drawn in an ellipse. The bounding box of the ellipse is used for the layout:

Text Alignment

Positions text relative to the selected bounding box or material size with options for left, center and right aligned.

Bounding Box Dimensions

These are the actual size of the box into which the text will be fitted. If the text is scaled interactively (by left clicking twice on the text) or precisely using the scale tool, the new bounding box is updated and displayed as a light gray rectangle.

Margin Size

The distance between the text and the bounding box where:

  • None - Scales text to fit the rectangle width or height of the bounding box
  • Normal - Scales text to fit within 80% of the bounding leaving a 10% border to the left and right.
  • Wide - Reduces the size to 60% of the rectangle width leaving a 20% border to the left and right.

Vertical Stretch

When the text fits the width of the box and there is space above and below it, the text can be made to fill that vertical space using one these methods:

No Vertical Stretch
No Vertical Stretch
Stretch Line Space to fit
Stretch Line Space to fit
Stretch Characters to fit
Stretch Characters to fit

Horizontal Stretch

When the text fits the height of the box and there is space at the sides, the text can be made to fill that horizontal space using one these methods:

No Horizontal Stretch
No Horizontal Stretch
Stretch Spaces between words
Stretch Spaces between words
Stretch Kerning (space between letters)
Stretch Kerning (space between letters)
Stretch Character size
Stretch Character size

Edit Text

To edit text properties or content of previously created text:
If the Create Text form is open, click the text you wish to edit or
If the Create Text form is closed, click the left mouse button on the text in the 2D View to select it before opening this form. The form will now allow you to edit the properties of the selected text.

Drawing | Circular Copy

This tool will automatically create a repeating pattern by making copies of the selected object and positioning them around a full or partial circle. The number of copies to be made can be entered directly.

Selected Objects Size

Reports the current size of the selection that you are intending to copy. This is for information only, but the values can be selected, copied and pasted to use in other calculations.

Rotation Center

This is the absolute XY coordinate around which the objects will be rotated when copied and pasted. The default Rotation point is the middle of the selection. You can set the rotation center coordinates explicitly using the X and Y edit boxes on this form or by clicking the selected geometry to show the transform grips, then double-clicking the center one to show the pivot-point and dragging the Pivot Point handle associated with the selection in the 2D View:

Rotate Copies

This option controls whether the copied objects are each rotated as they are placed around the circle, as shown in the diagrams below. If this option is selected, each copy is rotated according to its position on the circle. If the option is not selected then each copy maintains the orientation of the originally selected object.

Rotate Copies selected
Rotate Copies selected
Rotate Copies not selected
Rotate Copies not selected

Angle

Total Angle

With this option selected the number of items is divided into the Total Angle to give the incremental angle between each object.

Step Angle

With this option selected this angle is used to copy the selected vector(s) by this angle x the number of Items.

Note

A negative step angle pastes the copies in a counter-clockwise direction. A positive step angle pastes in a clockwise direction.

Drawing | Convert text to Curves

Converts selected text object into vector form, creating lines, arcs and Bezier spans that can be interactively edited. After conversion the text cannot be edited as a text object.

In most cases all the text created in Cut2D Pro can be Engraved, Pocketed and Profile machined without converting to the curves.

Some fonts do occasionally include loops and problems that need fixing using the Node Editing tools before it can be utilized for other functions.

Drawing | Copy Along Vectors

This tool automatically creates repeating patterns of objects by placing copies of them along the length of one or more selected vectors. The tool allows any existing object to be used but it also has an option specifically for the creation of circles, which is a common design element for patterns of this sort.

Copy Object

Any shape vector or group of vectors can be copied along a curve or curves. The first vector or group of vectors selected is the object that gets copied multiple times along the curves.

Copy Circles

Enter the diameter of the required circles

Selected Vectors
Selected Vectors
Circles Copied along curves
Circles Copied along curves

Distance between copies

This is the distance along the selected curve between each pasted vector. The Force even spacing option ensures that objects are pasted at the end points on the curve(s). If this option is not selected the pasted objects will be placed at the specified distance and may not match the exact length of the curve.

Number of copies

Selecting a specific number of copies automatically sets the specified number of copies along the entire length with an even spacing between them

Align Objects to curve

With this option selected the pasted objects are automatically aligned 'normal' or perpendicular to the curve they are being copied onto. If this is not selected, the copied objects stay in the orientation of the original.

Selected Vectors
Selected Vectors
Stars Copied along the curve
Stars Copied along the curve

Create Copies on new layer

This option creates the multiple copies on a new layer making it much easier to select and organize the resulting vectors for machining purposes etc.

Reverse Direction

If your copies appear upside down, this option will perform the copy operation in the opposite direction along the selected vectors and the resulting copied shapes will be created the other way up.

Drawing | Copy Operation

The Copy tool copies selected objects to the clipboard, leaving the original in place and allows duplicates to be made and re-used in the design by pressing the Paste icon. Only one item can be Cut or Copied at a time.

Drawing | Create Fillets

Fillets or radiuses can be added interactively at points where any two spans on a contour meet.

Creating Fillets

To use the filleting tool we select the icon from the drawing tab. Choose a radius for the fillet and the type of fillet you would like to use.

When the mouse cursor is near a node that can be filletted, the mouse cursor changes to show a check-mark ✓:

[object Object]
When the check-mark ✓ is visible, click the left mouse button to fillet the corner

Fillet Type

Normal Fillet

This creates a standard corner fillet based on the Radius defined, typically this would be used for design purposes and not for editing a slot for fitting purposes. Below left the image shows the vector before filleting the two inside radii, on the right is the filleted version

Straight Line Span Vectors before Filleting
Straight Line Span Vectors before Filleting
Straight Line Span Vectors After Filleting
Straight Line Span Vectors After Filleting

Dog-Bone Fillet

This creates a circular cut-out style of fillet, the circles will be placed so the upper right part of the circle touches the original sharp corner and are created with the Radius specified. This option should not be used if the slot width and the tool are similar in size. Below left is the vector showing the slot before filleting, on the right is the filleted version using the 'Dog-Bone' option.

Vectors before Dog-Bone Filleting
Vectors before Dog-Bone Filleting
Vectors after Dog-Bone Filleting
Vectors after Dog-Bone Filleting

T-Bone Fillet

This creates a circular cut-out style of fillet, the circles will be created with the Radius specified. This option should be used if the slot width and the tool are similar in size so the slot can grow out to the side to ensure there is space for them to fit. Below left is the vector showing the slot before filleting, on the right is the filleted version using the 'T-Bone' option.

Vectors before T-Bone Filleting
Vectors before T-Bone Filleting
Vectors after T-Bone Filleting
Vectors after T-Bone Filleting

The placement of the fillet is an interactive process; you can choose which side of the 'corner' the T-bone filet is placed. If you click on a 'corner' the fillet will be placed automatically on the longest side. By clicking to the side of the corner you want the fillet placed you can choose which side the fillet is placed on.

vertical edge clicked near the corner
vertical edge clicked near the corner
Horizontal edges clicked near the corner
Horizontal edges clicked near the corner

Removing Fillets

Fillets can be removed in the same way that we add fillets: move the cursor over the fillet that you wish to remove.
If this fillet can be removed then the cursor shows a cross to indicate that it is possible to remove a fillet:

Clicking removes the fillet:

Before removing fillet
Before removing fillet
After removing fillet
After removing fillet

When removing fillets the software does not store what kind of geometry the fillet was created from. It always defaults to using straight lines to return the fillet to a sharp corner. As such if the fillet is across multiple spans or is derived from arcs or Bezier curves then it will not go back to its original state and instead it will remove the radius and extend two straight lines to create the new corner.

Original Vector
Original Vector
Vector with Fillets
Vector with Fillets
New Vector after Removing Fillet
New Vector after Removing Fillet

Drawing | Create Text

This form allows text to be created at any height using the units the model is being designed in.

Entering Text

To enter text:

  • Click in the 2D view to choose the anchor position
  • Enter the text in the Text box
  • Edit the styling options. All changes are automatically applied

Font Selection

Vertical Fonts

Fonts that start with the @ character are drawn vertically downwards and are always left justified.

Engraving Fonts

The Single Line Radio Button changes the Fonts list to show a selection of fonts that are very quick to engrave.

Text Alignment

Positions text relative to the full body of text, this only has a noticeable effect when writing multiple lines of text.

Anchor

Sets the position of your text block. Either enter values directly, or use the mouse cursor to set the position values interactively:

  • For new text simply left click in 2D view in the desired location
  • For existing text object, left click the anchor point handle and drag it to the desired location

Editing Text

To edit text properties or content of previously created text:

  • If the Create Text form is open, click the text you wish to edit or
  • If the Create Text form is closed, click the left mouse button on the text in the 2D View to select it before opening this form. The form will now allow you to edit the properties of the selected text.

Drawing | Create a New File

This option opens the Job Setup form, which is used to create a new blank job of the specified dimensions and type. The relative origins for X0, Y0 and Z0 are also specified at this point, and the measurement units can be set in either inches or metric. The Modeling Resolution and default 3D shading color/material can also be set at this stage.

Drawing | Crop Bitmap

Select the image you would like to crop. Then using shift + left click select the closed vectors you would like to use to crop the image. You may select multiple vectors but the image must be selected first. Click the crop bitmap button to clear the image outside of the vector. If multiple vectors are used for the cropping then the crop tool leaves only the area of the image that lies inside the selected contours.

Drawing | Cut Operation

The Cut tool removes the selected objects from a design in a similar way to pressing the Delete key, but the selected objects are copied to the clipboard and can be Pasted into either the current file or a new file if required. Only one item can be Cut or Copied at a time.

Drawing | Dimensions

This tool allows you to add a variety of dimensioning annotations to your vector drawing.

Creating Dimensions

Unless specified separately below, the dimensions are created using these steps:

  • Select the dimension type you wish to need: length; height; width; angle or the radius or diameter of an arc.
  • In the 2D View, click with the left mouse button to set the points the dimension needs:
    For an Angle Dimension, the first point is the centre-point.
  • Click where you need the arrow-tips to be.
  • Click to set the location of the dimension-line.
  • Click to set where the annotation text will appear.

Editing Existing Dimensions

To edit an existing dimension while the form is open, hold down a Shift key while selecting it

Dimension Types

The dimension tool supports a number of different dimension types.

Length Dimension

Use this to dimension a straight-line length in any orientation between two points.

The text preview box will snap to to the middle of the dimension line, unless a Shift key is held down while dragging.

Vertical / Horizontal Dimension

These two options also allow any two points to be selected, but the resulting dimension will be locked to indicate a vertical or horizontal distance (respectively) between the two points.

The text preview box will snap to to the middle of the dimension line, unless a Shift key is held down while dragging.

Angle Dimension

This option allows any arbitrary angle to be measured. The process is similar to creating a 3 point arc. First you must pick the center of an angle you wish to measure - typically a corner point. The next 2 points clicked will set the extents of the sweep you are measuring. The next Click will determine the dashed dimension line positioning and the final click will set the position of the text annotation.

  • Angle Dimensions' arrow-heads will pop outside small angles if there is not room to draw them inside.
  • Angles are extended with a dashed extension-line where required, allowing the dimension to be placed anywhere. The text snaps to the angle center and the leader-line angle snaps to horizontal, vertical or diagonal (disable snapping by holding down a Shift key).
  • Angle Dimensions use a separate Decimal Places value to the other dimensions (as you change dimension-type you may notice the Decimal Places value change).
  • Angle dimensions can now have up to six decimal places.

Arc Dimension

With this option selected you will only be able to select arc spans with the first click of dimension tool (Bezier curve spans are not supported). The second click will set the position of the dimension annotation, which will show the radius (or diameter) of the selected arc span.

  • To display the diameter of an arc dimension simply check ✓ the Show Diameter box.
  • Arc Dimensions recognise when a circle has been selected and allow placement anywhere around the circle. Arcs will now be extended with a dashed extension-line where required, allowing the dimension to be placed anywhere. The text snaps to the arc/circle center and the leader-line angle snaps to horizontal, vertical or diagonal (disable snapping by holding down a Shift key).

Note

Circles or arcs that are polygonized (from an imported file or from the Curve fit vectors command using Straight lines) are not recognized and cannot be dimensioned with this tool

Font Selection and Settings

This section of the form allows the user to change the settings for the dimension annotation, such as the font to be used, the height of the text and how many decimal places are required. The Offset field determines the gap left between the dimension markers and the vectors that are being measured.

Use Custom Text

You can check ✓ Use Custom Text to insert your own custom text. The text is stored per dimension, so you change between calculated and custom text without losing a dimension's custom text. When the form is first opened it defaults to calculated text.

Place Dimensions on Layer

By default this option is checked ✓ and the dimensions will be placed on a mid-gray Dimensions Layer. You can edit the name of the layer in the Name edit field. If a layer of this name does not exist, it will be created automatically.

Note

Dimensions can be edited. Hold shift while selecting the dimension you wish to edit or use the Undo shortcut Ctrl+Z to undo previously created Dimensions while still in the Dimensioning tool.

Drawing | Distort Object

This tool allows you to bend and flex a vector or component by manipulating a distortion envelope using standard node editing tools. You can select one or more vectors or components and then use one of the three different tool modes to create your initial distortion envelope.

Multiple Objects

You can distort several vectors or components at once but you cannot distort a mixture of vectors and components together in a single operation.

Once the distortion envelope has been created, you can use the node editing tools to add or edit its nodes and spans. As you alter the shape of the envelope the associated object will be distorted to reflect the changes.

Layers

When distorting a selection of objects which fall on different layers, the result will be created on the layer of the first object in the selection.

Use Rotated Bounds

This option is only supported if you only have one object selected to distort. It makes use of the local rotation of the object as shown in the Selection Tool.

When this option is ticked,

  • The initial distortion envelope is created along the transformed bounds of the selected object.
  • When distorting along a curve (or two), the object is distorted on the curve in its local transformation. This is useful if you're distorting a rotated object onto a rotated curve, for example.

Bounding Box Distortion

This option is available if you have a selection of vectors or components (Note that you cannot mix vectors and components in this mode). It creates a distortion envelope based on the closest bounding box that can be drawn around your selection. Thus the resulting envelope is always initially a rectangle, comprising four line spans and a node at each corner. Using the normal node editing tools, however, you can modify this envelope as much as you like and the shape within it will be distorted accordingly.

Along a Single Curve

This option is only available if the last item in your selection is an open vector that can be used to define a curve, above which the other selected objects will be distorted. The distorted object can comprise one or more vectors or one or more components, but not both.

Using this option, you will usually end up with your objects bent to match the curve in your original selection. The distortion curve itself is left unchanged by this operation.

Between Two Curves

This option will become available if the last two objects in the current selection are open vectors, between which the other objects can be distorted.

Baking Distortion into an Object

Once an object has been distorted, node editing will always relate to the object's distortion envelope. If you wish to edit a distorted vector directly again, you will first need to permanently apply the distortion to the shape.

If you select an object that already has a distortion envelope while in the Distort Object tool, the button will be available. Clicking this button will permanently apply your current distortion and you will then be able to either distort the object again (with new settings), or node edit the shape directly.

Drawing | Draw Arc

The Create Arc tool allows a single arc span to be created using precise values, or dynamically within the 2D View.

Through 3 Points

  • Left click the mouse in the 2D View to set the start point of an arc.
  • Click again to set the end point position.
  • Move the mouse and click a third point to set the arc's radius.

Center, Start and End

  • Left click the mouse in the 2D View to set the center point of the arc.
  • Click again to set the start point of the arc.
  • Move the mouse and click a third point to set the end point of the arc.

Note

Clicking the Right mouse button or pressing the Esc key will complete the arc drawing if possible and close the form.

Exact Size

Precise values for the start and end point positions (in absolute X Y coordinates) and either the radius or the height of the arc can be entered in the form directly. Click to draw and arc using these values.

Editing An Existing Arc

The properties of an arc can be edited at any time by selecting the arc before choosing the Create Arc tool.

This opens the form with the current properties and position of the selected arc and these values can then be edited.

Click to update the selected arc with the new values.


Drawing | Draw Circle

Circles can be created interactively with the cursor and Quick Keys or by entering the exact coordinates and diameter / radius with typed input.

Note

Pressing the Space-bar re-opens the last vector creation form you used. This is very useful when using other forms in between each shape you create.

Interactive

Cursor

The default mode and the procedure for drawing circle is:
Click and drag the Left mouse to indicate the center point followed by releasing the button at the required radius / diameter (depends on what is set on the form).

Note

Holding Alt and dragging creates a circle from the middlepoint.

As the cursor is dragged across the screen the radius is dynamically updated. The increments will depend upon your snap radius and the job size.

Quick Keys

The radius or diameter can be specified while dragging out a circle:

Type the value while dragging followed, by D if it's a diameter, or R if it's a radius:

Example:

1 2 R Gives a radius of 12

Exact Size

Circles can also be drawn by entering the required XY origin, selecting either Radius or Diameter and entering the required size on the form.

Click to update the circle.

Edit

Open the Draw Circle form and select the circle to modify.

The selected circle is displayed as a dotted magenta line. Edit the Center Point and Radius or Diameter

Click to update the circle

To modify another circle without closing the form hold a Shift key down and select the next circle.

Close the form

To finish drawing with the tool, you can:

  • Click on the form
  • Press the Esc Key
  • Click the Right mouse button in the 2D View

Drawing | Draw Curve

This tool creates a smooth, flowing, continuous curve through clicked points.

Form

Draw Curve does not require an associated form, just use the mouse cursor directly within the 2D View.

Controls

  • Click in the 2D View to begin drawing at the clicked point.
  • Move the mouse pointer within the 2D View and click the left button to insert as many points as you require. A curve will be created that smoothly joins your points.
  • Click the right mouse button or press Esc to finish drawing your curve and close the tool.
  • Alternatively, press Space Bar to finish drawing one curve, but keep the tool active so that you can immediately begin drawing another curve.

Left Clicking

Left clicking when the mouse pointer is close to the first point on the curve will snap the curve closed.

Extending Contours

An existing open contour can be extended by holding down the Ctrl key and then clicking on either its start or end point.

CTRL clicking on the start point of a contour will cause the contour to be reversed before extending.

Drawing | Draw Ellipse

Ellipse / ovals can be created interactively with the cursor and Quick Keys or by entering the exact coordinates for the center point, height and width with typed input.

Note

Pressing the Space-bar re-opens the last vector creation form you used. This is very useful when using other forms in between each shape you create.

Interactive - Cursor

The quickest and simplest way to draw an ellipse is:

  • Click and drag the left mouse button in the 2D View to begin drawing the ellipse from its corner.
  • While holding the left mouse button, drag to the required size.
  • Releasing the left mouse button.
  • Holding Alt and dragging creates an ellipse from the middle point.
  • Holding Ctrl and dragging creates a circle.

Quick Keys

Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.

  • Left-click and drag out your shape in the 2D View.
  • With the left mouse button still pressed, enter a quick key sequence detailed below.
  • Release the left mouse button.

Default

By default, two values separated by a comma, will be used to set width and height of your ellipse. One value will create a circle with the given diameter. While you are dragging out the ellipse, type Width Value , Height Value Enter or Diameter , Enter to create an ellipse with the specified dimensions.

Specifying Further Properties

By using specific letter keys after your value, you can also indicate precisely which property it relates to.

  • Value X - Creates an ellipse at current dragged height but with set width
  • Value Y - Creates and ellipse at current dragged width but set height
  • Value W Value H - Creates an ellipse with set width and height

Examples

  • 1 x Current dragged height with width (X) of 1
  • 1 y Current dragged width and height (Y) of 1.

Exact Size

Accurate ellipses can also be drawn by entering the required XY origin point with the Width and Height of the oval. Click to create the ellipse.

Editing an Ellipse

To edit an existing ellipse:

  • Select the ellipse to modify and open the Draw Ellipse form.
  • The selected shape is displayed as a dotted magenta line.
  • Edit the Width and Height values.
  • Click to update the ellipse.

To modify another ellipse without closing the form hold a Shift key down and select the next ellipse.

Drawing | Draw Line

This tool creates continuous straight lines through points clicked, entered coordinates, tangent between a point and an arc or tangent to two arcs.

Interactive - Cursor

The quickest and easiest way to draw a line is by clicking within the 2D View using the mouse.

  • Click the left mouse button to indicate the start point of your line.
  • Move the mouse pointer and click again to set the next point in your line.
  • Repeat this process to add as many line segments as you require.
  • Right-click or press Esc to finish your polyline and exit the form.
  • Alternatively press the Space bar to complete this polyline but keep the form open and begin drawing another polyline.
  • Press the Tab key to automatically close the vector.

Creating Tangent Lines

The polyline tool can also be used create lines that are tangent to arcs in your existing drawing.

From A Point To An Arc

To create a line tangent from a point to an arc simply enter the initial point and then hover the cursor over the arc and press T.

From An Arc To A Point

To create a line tangent from an arc to a point click on the arc to insert a point and then hover the cursor over the next point position and press T

Note

You cannot create a tangent line to a bezier curve

From An Arc To Another Arc

To create a line tangent from one arc to another click on the arc to insert a point and then hover the cursor over the second arc and press T.

Note

Arcs are not trimmed as a result of creating a tangent line

Quick Keys

Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.

  • Left-click and drag out your shape in the 2D View.
  • With the left mouse button still pressed, enter a quick key sequence detailed below.
  • Release the left mouse button.

By default, entering a single value will be used to add a point at the specified distance along the line direction currently indicated by the mouse pointer position, relative to the preceding point. With polyline drawing underway, move the mouse pointer in the direction you wish to create a new line segment and type Length Value Enter to extend the line by the specified distance in that direction.

By default two values, separated by a comma, will create the next line point at the absolute X Y coordinate indicated by the two values, respectively. While drawing, type X Value , Y Value Enter to place the next point precisely at specified X and Y position

Examples

  • 3 . 5 Enter - Adds the next point at a distance of 3.5 along the line direction indicated by current mouse direction
  • 1 , 2 . 5 Enter - Adds the next point at the absolute position 1 in X and 2.5 in Y

Specifying Further Properties

By using specific letter keys after your values, you can also specify the line segment in terms of angle and length. Using the key sequence value A value L cretes the next line segment at angle (A) degrees from the last point and with a length(L)

Examples

  • 45 A 3 L - Creates a line segment at 45 degrees and length 3

Next Point

You can also use the form to enter values for each line segment as you go along. The segments can be defined using:

  • The absolute X Y position of the next point
  • The Angle and Length to the next point
  • The relative offset in X (dx) and Y (dy) to the next point.

Once you have entered the values you wish to use:

  • Click the button to enter a new point.
  • The button deletes the last point entered and allows a new point to be added.
  • The button completes drawing the current line and leaves the form open to allow additional lines to be drawn.

Note

The X Y position use absolute coordinates. The Angle, Length and dx/dy positions are incremental from the current position.

Drawing | Draw Polygon

Polygons (e.g. Triangles, Pentagons, Hexagons etc.) can be created interactively with the cursor and Quick Keys or by entering the number of sides, exact coordinates and radius using typed input.

Interactive Creation

The quickest and easiest way to draw a polygon is by using the mouse in the 2D View.

  • Click and hold the left mouse button to indicate the center point.
  • Drag the mouse while holding down the left mouse to required radius.
  • Release the left mouse button to complete the shape.

Note

Holding ALT and dragging creates a polygon from the middle point.

Quick Keys

values during the dragging process and set properties precisely.

  • Left-click and drag out your shape in the 2D View.
  • With the left mouse button still pressed, enter a quick key sequence detailed below.
  • Release the left mouse button.

Default

By default, entering a single values will be used to set the radius of your polygon. While you are dragging out the polygon, type Radius Value Enter to create a polygon with the precisely specified radius.

Example

  • 2 . 5 Enter - Creates a polygon with a radius of 2.5. All other settings as per the form

Specifying Further Properties

By using specific letter keys after your value, you can also indicate precisely which property it relates to.

  • Value D - Creates a polygon with the diameter specified, with all other properties as per the form.
  • Value S Value R - Create a polygon with the specified number of sides (S) and the outer radius (R)
  • Value S Value D - Creates a polygon with the specified number of sides (S) and the outer diameter (D)

Examples

  • 1 R - Outer radius 1, number of sides as per form
  • 1 D - Outer diameter 1, number of sides as per form
  • 8 S 1 R - An 8 sided polygon with outer radius R of 1
  • 6 S 2 . 5 D - A 6 sided polyon with an outer diameter of 2.5

Exact Size

Polygons can also be drawn by entering the required XY origin , selecting either Radius or Diameter and entering the required size.

Click to update the circle

Editing Existing Polygons

To edit an existing polygon select the polygon, edit the parameters and click to update the circle.

Drawing | Draw Rectangle

Rectangles can be created by using the Draw Polyline tool or using the Draw Rectangle Tool. The latter tool allows rectangles to be created interactively with the cursor and Quick Keys or by entering the exact coordinates, type of corners (square, internal or external radius) and Width and Height using typed input.

Interactive Creation

The quickest and simplest way to draw a rectangle is:

  • Click and drag the left mouse button in the 2D View to begin drawing the rectangle from its first corner.
  • While holding the left mouse button, drag to the required size.
  • Releasing the left mouse button.

Note

Holding Alt and dragging creates a rectangle from the center. Holding Ctrl creates a square.

Quick Keys

Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.

  • Left-click and drag out your shape in the 2D View.
  • With the left mouse button still pressed, enter a quick key sequence detailed below.
  • Release the left mouse button.

Default

By default, two values separated by a comma, will be used to set width and height of your rectangle. One value will create a square with that side length. While you are dragging out the rectangle corner, type Width Value , Height Value Enter or Side Length , Enter to create a rectangle with the specified width and height.

Example

  • 1 , 2 . 5 Enter - Creates a rectangle of width 1 and height 2.5

Specifying Further Properties

By using specific letter keys after your value, you can also indicate precisely which property it relates to.

  • Value X - Creates a rectangle at the dragged height but with the width set to the entered value
  • Value Y - Creates a rectangle at the dragged width but with the height set to the entered value
  • Value R Value X - Create a rectangle with radius R and width X
  • Value R Value Y - Create a rectangle with radius R and height Y
  • Value W Value H - Create a rectangle with width W and height H
  • Value R Value W Value H - Create a rectangle with width W and height H

Examples

  • 1 X - Current dragged height with a width of 1
  • 1 Y - Current dragged width with a height of 1
  • 0 . 1 R 1 X - A corner radius of 0.1, a width of 1 and current dragged height
  • 0 . 1 R 1 Y - A corner radius of 0.1, a width of 1 and current dragged height

Note

These key combinations must be pressed whilst dragging with the mouse to create the rectangle.

Exact Size

Rectangles can also be drawn by entering the required XY origin point with the Width and Height of the rectangle.

Corner Type

Corners of the rectangle can be Square, Radiused Externally or Radiused Internally.

Editing Existing Rectangles

To edit an existing rectangle:

  • Select the rectangle to modify and open the Draw Rectangle form.
  • The selected shape is displayed as a dotted magenta line.
  • Edit the Width and Height values.
  • Click Apply to update the rectangle.

To modify another rectangle without closing the form hold a Shift key down and select the next rectangle.

Drawing | Draw Star

Stars can be created interactively with the cursor and Quick Keys, or by entering the number of points, exact coordinates and outer radius and inner radius percentage using typed input.

Interactive Creation

The quickest and easiest way to create a star is by clicking and dragging the shape to size in the 2D View using the mouse.

  • Click and hold the left mouse button to indicate the center point.
  • Drag the mouse while holding down the left mouse to required radius.
  • Release the left mouse button to complete the shape.

Note

Holding Alt and dragging creates a star from the middle point.

As the cursor is dragged across the screen so the outer radius is dynamically updated. The increments will depend upon your snap radius and the job size.


Quick Keys

Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.

  • Left-click and drag out your shape in the 2D View.
  • With the left mouse button still pressed, enter a quick key sequence detailed below.
  • Release the left mouse button.

Default

By default, entering a single value will be used to set the outer radius of your star. While you are dragging out the star, type Radius Value Enter to create a star with the precisely specified outer radius.

Example

  • 2 . 5 Enter - Creates a start with an outer radius of 2.5 all other settings as per the form

Specifying Further Properties

By using specific letter keys after your value, you can also indicate precisely which property it relates to.

Note

When specifying multiple properties with quick keys, it is still important that they are entered in the order indicated in the table below.

  • Value D - Creates a start with the outer Diameter (D) specified with all other properties as per the form
  • Value I Value R - Creates a star with the inner radius percentage (I) and the outer radius (R). The inner radius is defined in terms of a percentage of the outer radius or diameter. All other properties are as per the form.
  • Value P Value R - Creates a star with the specified number of points (P) and the outer radius (R).
  • Value P Value I - Creates a star with the specified number of points (P), inner radius percentage (I) and the outer radius (R).

Examples

  • 1 R - Outer radius 1, other properties as per form
  • 1 D - Outer diameter 1, other properties as per form
  • 6 P 1 R - A 6 pointed star with an outer radius of 1
  • 6 P 2 5 I 4 D - A 6 pointer (P) star with an outer diameter (D) of 4 and an inner diameter that is 25% of the outer (i.e. 1).

Exact Size

Stars can also be drawn by entering the Number of Points, Center Point, Outer Radius and Inner Radius Percentage.

  • Click to update the star.

Editing an existing star

To modify an existing star:

  • Select the star to modify and open the Draw Star form.

The selected shape is displayed as a dotted magenta line.

  • Edit the required parameters.
  • Click Apply to update the star.

To modify another star without closing the form hold a Shift key down and select the next star.

Drawing | Edit Picture

The Edit Picture form allows you to add a border to, and edit the properties of a selected bitmap.

Contrast

This slider adjusts the contrast. A higher contrast emphasises the differences between the light and dark parts of the image.

Brightness

This slider adjusts the brightness of the image.

Gamma

This slider adjusts the gamma correction applied to the image. This can make an image look lighter or darker whilst maintaining detail.

Invert

Inverts the colors in the image. White becomes black and black becomes white

Grayscale

Makes the image black and white.

Add Border

Fades the edges of the image based on the border type and the width of the fading.

Rectangular Border
Rectangular Border
Oval Border
Oval Border

Drawing | Extend Vectors

This tool allows you to extend two vector lines to their common point of intersection.

With the Extend Vectors tool active, moving the mouse pointer over the ends of open vector shapes (without clicking) will highlight a dashed preview extension line from that shape. The line will change dynamically as you move the mouse over the end spans of different open shapes. Clicking with the left mouse button at this point will set it as the target line to extend and the magenta line will remain visible.

The mouse can now be moved over existing spans along the length of the preview extension line, or over the end of another shape to create a second, intersecting, preview extension line.

Clicking on any of the intersection points indicated by the mouse cursor will extend the initial shape to that point and complete the operation.

First click creates a preview extension line from the selected vector span.
First click creates a preview extension line from the selected vector span.
Moving the mouse over another span will display a second preview extension line to the point of intersection. Click the line to apply this change.
Moving the mouse over another span will display a second preview extension line to the point of intersection. Click the line to apply this change.

The tool can be closed at any time using the button on the form. Right-clicking in the 2D View will reset the tool so that it is ready to select another target line to extend.

Drawing | Fit Curves To Vectors

This function allows the user to fit arc, Bezier curves or straight lines to selected vectors. The newly created vectors will be approximated based on a user defined tolerance. Using this function can aid with smoothness for some toolpath options and also help to simplify data for modeling purposes.

Fitting Type

Circular Arcs

Checking ✓ this option means the selected vectors will be approximated using arcs:

Before Fitting
Before Fitting
After fitting
After fitting

Bezier Curves

Checking ✓ this option means the selected vectors will be approximated using Bezier curves.

Fitted with Bezier spans
Fitted with Bezier spans
The same bezier spans in Node-edit mode
The same bezier spans in Node-edit mode

Straight Lines

Checking ✓ this option means the selected vectors will be approximated using straight lines.

The vector before fitting
The vector before fitting
The same vector fitted with straight lines
The same vector fitted with straight lines

Tolerance

The value which is set in the Tolerance area determines how closely the original vectors will be approximated. The newly created, Arcs, Beziers or Lines will be generated within a distance of the original vector which is plus or minus the specified Tolerance value. The smaller the value the closer to the original the new data will be but it will also mean more data points will be used. A larger Tolerance will not be as accurate to the original but will have less data points.

Keep Sharp Corners

Checking ✓ this option will make the Curve Fitting routine keep sharp corners which have a difference greater than the Max Angle value specified. Any corners where the difference in angle is less than this value will be modified within the specified tolerance.

Initial Vectors
Initial Vectors
Result after Keep Sharp Corners
Result after Keep Sharp Corners (max. angle = 20 degrees)

Replace selected vectors

Checking ✓ this option will delete the current vectors and replace them with the new curve fitted vectors. Un-checking it will keep the original vectors as is and in addition create new curve fitted vectors. The new vectors will always be created on the currently selected Layer.

Drawing | Group Selected Objects

Vectors can be Grouped allowing any number of vectors to be included as a single object that can easily be selected, moved and scaled etc. The Shortcut key for this operation is G.

Grouping vectors is particularly useful for machining purposes, where different vectors will be used for a single toolpath operation. Clicking any member of the group will select the entire group.

Drawing | Grouping and Ungrouping

Grouping objects allows you to select, move and manipulate them as if they were one entity. The process is entirely reversible by Ungrouping.

See Grouping and UnGrouping.

Drawing | Import Bitmap

This opens the File Open dialog window and allows image files to be selected and imported into the current open job. File types - BMP, JPG, TIF, GIF, PNG

Images are imported to sketch vectors over the top of them, generate traced vectors or to be used to generate a 3D Component directly from the image. These functions will be covered in more detail in the

Drawing | Import Vectors

This opens the File Open dialog window and allows 2D DXF, EPS and AI and PDF files to be imported into the 2D View. The imported vectors will always be read in at the size and scale they were created in their original design software. Once open they can be scaled and edited in the same way as vectors created in Aspire. All the Vector tools will be dealt with in that section of this manual.

To import toolpaths from PhotoVCarve and Cut3D (.PVC and .V3D file extensions), use File ► Import... ► Import PhotoVCarve or Cut3D Toolpaths from the file menu bar. Any Toolpath data saved as .PVC or .V3D files can be imported and will be visible in the Toolpath List.

See the 3D Toolpath Files section for detailed instructions on importing PhotoVCarve(*.pvc), Cut3D(*.v3d) or Vectric 3D Machinist(*.v3m) files.

Drawing | Interactive Selection Mode

The Interactive Move, Rotate, Scale Selection tools can be used to quickly and easily modify vectors and components.

Clicking twice on one of the selected objects and the interactive scaling, movement and rotation handles are displayed in the same way as selecting this icon. Lines, Arcs and Bezier spans will be displayed as dotted magenta lines and text and grouped objects will be displayed as solid magenta lines:

When in this mode the mouse is used to click on one of the handles which has appeared on the selected Vector/s. Each handle is used for a specific editing operation as detailed here:

  • Middle - Move the vectors (Or +Alt Move the selected objects in one axis)
  • Corner (White) - Scale the vectors proportionally (Or +Alt Scaling non-proportionally, +Shift Scale around the centre)
  • Edges (White) - Scale the vector in one axis (Or +Shift Scaling proportionally)
  • Corner (Black) - Rotate the vectors (Or +Alt Rotate in 15° increments)

To deselect objects,

  • Click the white background unless Shift is pressed.
  • Press Esc
  • Right click menu ► Unselect All

Drawing | Interactive Vector Trim

The interactive trimming tool allows the user to just click on sections of vectors they want to delete.

The program finds the closest intersections either side of the clicked portion of the vector and removes the piece of the vector between the intersections. Optionally, when the form for this command is closed, the program can rejoin all the remaining trimmed pieces automatically.

Without using this tool, to remove an overlapping section of a vector, the user would need to insert extra nodes into both vectors, manually delete the intermediate sections and then manually join the resulting pieces. These operations can be performed with a single click using this tool.

When the tool is selected the cursor changes into a 'closed' scissor shape. When the cursor is moved over a vector suitable for trimming the scissors 'open' to show you can click and trim.

Rejoin Trimmed Sections

Allows the user to select whether the program will automatically try to rejoin trimmed vectors when the form is closed. For most simple cases like that shown above with the overlapping rings, this option can be left checked ✓. If you have an example where for instance many trimmed lines meet at the same point, you may want to uncheck this option and rejoin the vectors manually.

Drawing | Join / Close Vector with a Smooth Curve

Join with a Curve finds the closest end points on 2 selected, open vectors and joins them together with a smooth curve.

Cut2D Pro has two smooth joining methods:

  • A smoother method (new for V9.5)
  • A more symmetrical shallower join method
Example of smoother joining (left) versus symmetrical joining (right)

Drawing | Join / Close Vector with a Straight Line

Join with a Line finds the closest end points on 2 selected, open vectors and joins with a straight line. Close with a Line closes a single open vector with a straight line between its two end points.

Drawing | Join Open Vectors

The icons to join and close vectors are located under the Edit Vectors section of the Drawing Tab.

Open vectors are automatically identified and closed or joined to other vectors where the end points lie within the user definable tolerance.

Drawing | Join/Close by Moving End Points

Join Moving End Points finds the closest end points on 2 selected, open vectors, calculates the mid-point between them and moves the end points to this position.

Drawing | Measure - Inspect

The Measure tool allows you to find important information about your model or drawings.

Measure Between 2 Points

With this option selected, you can click on two points in the 2D View and the form will report the measurements between the clicked locations

Distance

Straight line distance between the two points.

Angle

The angle (in degrees) of the line joining the two points, where horizontal is zero degrees and vertical is ninety degrees.

X Distance

The separation between the two clicked points in X only.

Y Distance

The separation between the two clicked points in Y only.

First Point

The precise X and Y coordinates of the position first clicked.

Cursor Position

The dynamically updated coordinates of the mouse cursor position.

Span / Contour Properties

This mode allows you to find precise information about the individual spans of a vector shape in 2D View. Use your mouse pointer to click on any part of the shape and the information relating to the entity you have clicked will be displayed on the form.

Type

The type of span you have clicked.
Possibilities include:

  • Line
  • Arc
  • Bezier Curve

Length

The length of the clicked span.

Start Point and End Point

The precise coordinates of the node forming the start and end of the selected span.

Vector

Information relating to the whole vector, of which the selected span is part, is shown in this section.

Area

The total area of the selected vector

Perimeter

The total length of all the spans forming the perimeter of the shape

Num. Spans

The total number of spans in the shape.

Model Cross Section

The Model Cross Section option allows you to select two points on the 2D View and create a new vector that shows the corresponding cross-section of the underlying 3D model.

Drawing | Mirror

Selected vectors/bitmaps/component grayscale previews can be mirrored to a new orientation.

Selected objects can also be mirrored about axes of symmetry relative to the bounding box of the selection, using the standard options on the Mirror Form.

  • Select the object or objects to mirror.
  • Click on the Mirror icon to open the Mirror Form.
  • Select the Create a mirrored copy option to leave the selection and create a new set of objects.
  • Click the button to accept the changes.

Use Rotated Bounds

This option is available only when a single object is selected. When it's checked, it will flip the object around its local rotated bounds as shown in the Selection Tool. If the object isn't rotated, it will just operate normally.

Shortcuts

The following shortcuts can be:

  • H - Mirror Horizontally
  • Ctrl + H - Create mirror. Copy Horizontally
  • Shift + H - Mirror horizontally around center of material
  • Ctrl + Shift + H - Create mirror copy horizontally around center of material.
  • V - Mirror vertically
  • Ctrl + V - Create mirror. Copy Vertically
  • Shift + V - Mirror vertically around center of material
  • Ctrl + Shift + V - Create mirror copy vertically around center of material.

Drawing | Move Selection

Selected items can be accurately moved and positioned using this option.

Anchor

The anchor position determines the point on your selected object's bounding box that will be moved to the absolute position entered.

Type of Move

Absolute

In this mode, the X Position and Y Position values will be used to position the object's anchor point directly

Relative

With this option selected, the values entered in the X Position and Y Position fields will incrementally offset the object from its current position, by the distances entered. The Anchor options are not relevant in this mode and so will be disabled.

The keyboard shortcut M opens the Move form in interactive mode.

Drawing | Nest Parts

The Nesting tool will automatically fit vector shapes within the user defined area in the most efficient way it can calculate (based on the user defined parameters). By default the area the vectors will be fitted is the current Job Size but it is also possible to select a vector as the nesting area. This is a powerful way to optimize material usage and increase toolpath efficiency when laying out and cutting a number of shapes.

Object Selection

The Nesting tool allows you to select open vectors, closed vectors and text.

Once selected the objects will form parts, with part outer boundary highlighted with a thicker line.

The basis for forming parts is overlapping. If selected object contains another or overlaps with it they will be considered the same part.

Tool and Clearance Settings

The settings in this section of the form will determine the spacing which will be left between each of the nested vectors and also control how close they are to the edge of your nesting area.

Tool Dia. (D)

Enter the diameter of the tool that you will be using to Profile (cut-out) the vectors you are nesting. This is the minimum distance that will be left between shapes once they are nested.

Clearance (C)

The Clearance value will be combined with the specified Tool Diameter to create the final minimum spacing between the nested shapes. For example a Clearance of 0.05 inches combined with a Tool Diameter of 0.25 inches would create a minimum spacing gap of 0.3 inches (0.05 + 0.25 = 0.3).

Clearance less than Tool Diameter
Clearance less than Tool Diameter
Clearance greater than Tool Diameter
Clearance greater than Tool Diameter

Border Gap

The Border Gap value is applied to the edge of the area which is being used to nest the vectors into. It will be added to the Clearance value around the edge of this shape to create the minimum distance that parts will be nested in respect to the nesting boundary.

No Border Gap
No Border Gap
Border Gap
Border Gap

Part Nesting Options

The options in this area of the form will all directly affect how many parts or how efficiently it is possible for the software to fit shapes into the defined nesting area.

Rotate Parts to find best fit

Checking ✓ this option will allow the software to rotate the selected vectors in order to try and better fit them. The increments of rotation the software will use is based on the Rotation step angle.

Rotate Parts Enabled
Rotate Parts Enabled
Rotate Parts Disabled
Rotate Parts Disabled

Mirror parts to find best fit

Checking ✓ this option will allow the nesting to mirror (flip) the vectors in order to try and more efficiently nest the selected shapes. This should only be checked ✓ if the direction the parts are cut in is not important.

Allow parts inside other parts

Checking ✓ this option will allow the software to nest within the internal areas of shapes that have gaps in the middle.

When this option is active, the internal areas that will be considered in nesting will be highlighted.

Original
Original
Parts Nested inside other parts
Parts Nested inside other parts

Nest two-sided parts

This option is only available for double-sided projects and allows nesting on both sides simultaneously. When this option is active, any visible objects on the other side will be included, if they intersect with objects selected on active side.

When using this mode it is recommended to perform selection on the side that contains cut-out contours.

When part is selected, the included vectors on the other side will be highlighted as can be seen below.

Double-sided part - not selected
Double-sided part before selection
Double-sided part - selected
Double-sided part when selected

Sheet Options

Nest From

This area of the form is used to define which corner the nesting will start in. There are four options which can be selected from the options in the form.

Nest Direction

he options in this area of the form are used to select how the parts will progress as they are positioned within the sheet. The best way to think of this (for the purposes of this section) is that they 'pour' out of the selected corner filling the sheet in one axis then advancing along the other defined axis (X or Y) .

Along X
Along X
Along Y
Along Y

Last vector is nest boundary

Checking ✓ this option means the last vector selected will be used as the boundary for the nesting area. This can be useful if you need to define a non-rectangular shape to Nest Parts into, such as large off-cuts from a previous job. It's important to note that using this option will not respect the currently defined Job Area if the selected boundary vectors goes outside of it.

Note

If you need to represent a sheet with holes or other features which can't be represented with a single selected vector as the new boundary it is possible to also use a Grouped vector for the last selected item then the shapes will be nested within the spaces in this.

Individual Part Properties

If you want more than one incidence of a particular item then select it from the 2D view. In the box where it says Number of Copies enter as many copies as you want and hit and the selected vectors will be marked with a green number indicating how many copies of that item will be made when they are nested. Different shapes or groups of shapes can be assigned different numbers of copies. To stop an item being copied multiple times just set the Number of Copies back to 1 and click .

Active Sheet

This option lets you choose which Sheet of vectors is currently active, either for editing or applying toolpaths onto.

Drawing | Node Editing Mode

The Node Editing tool can be selected from the Editing window or by pressing the Keyboard shortcut N to toggle between Selection and Node Editing modes.

Vectors Selected
Bezier node editing

When the Node Editing tool is active the cursor changes to a Black Arrow indicating that individual points (nodes) and their connecting spans can be edited. Nodes can be interactively moved by clicking and dragging the left mouse button on a node to select and move the node to a new position.

The shape of lines, arcs and Bezier (curve) spans can be edited by clicking and dragging on the nodes or control points to move them. Multiple nodes and control points can be selected and moved by using the multiple selection options such as the Shift key and dragging to make a selection.

The shape of individual spans can also be edited by dragging the span itself using the left mouse button.

Holding down the Ctrl key while dragging an arc or Bezier span will move the entire span rather than change its shape.

The start and end directions of Bezier curves can be fixed when being dragged directly, by toggling on Keep Bezier Tangency mode.

If you right click on nodes or spans a context sensitive popup menu will be displayed which allows you to insert or delete points and nodes, cut the vector, move the start point, etc.

Node editing vectors is a very powerful way to be able to make changes to the vectors in your part.

Useful Tip

Smart Snapping combined with Distance Snapping or Quick Keys can give more accuracy when dragging nodes.

Drawing | Object Selection Tools

Once vectors have been created within Cut2D Pro or have been imported from other design software packages you may want to make changes to them. These changes may be to prepare for machining or for use as construction vectors for making 3D shapes using the Modeling Tools. There are a number of functions for editing vectors which will be covered in this section of the manual. All the icons under the Edit Vectors section of the Drawing Tab will be referenced along with the icons under the Align Objects section of the menu.

Editing Modes

From the 2D view a vector can be selected and then three different editing modes allow different dynamic edits to be made to the vector(s) depending on which option is selected from the Edit Vectors section.

The three editing modes are:

By default the software is normally in the Vector Selection mode.

Drawing | Offset Vectors

Selected vectors (open or closed) can be offset either inwards or outwards to create new vector shapes that might be useful for edge patterns or borders etc. To offset a vector shape, use the following steps:

  • Select the vectors to offset
  • Select the required direction - Outwards / Right or Inwards / Left
  • Enter the Distance
  • Click the button

Options

The offsetting options are slightly different in their behavior depending on whether the vector to be offset is open or closed. See below for more information.

Create sharp offset corners

Will retain any sharp corners in a design.

Offset with Sharp Corners on
Offset with Sharp Corners on
Offset with Sharp Corners off
Offset with Sharp Corners off

Offsetting Open Vectors

When offsetting open shapes, the options are either to the Right or Left side of the selection. The direction of open vector(s) is very important as this is used to decide the right and left side of the selection. Selecting Node Edit mode (pressing N on the keyboard) will display a Green node at the start of the vector. Looking along the vector(s) from the green node indicates the direction and the image below shows offsets to the left and right of an open vector.

[object Object]


Drawing | Open a File

This option opens the File Open dialog window, allowing Aspire files (CRV) and importable 2D vector files to be selected and opened.

Drawing | Overlap Vectors

Selected closed vectors that overlap can be merged together to create a new shape. These tools consider the closed vectors to be solid areas.

The following examples begin with these five vector shapes where the rectangle was selected last.

Only areas of the first selected parts (the circles) that are covered by the last selected vector (the rectangle) remain after this operation.

Drawing | Paste Operation

This Paste option places the contents of the clipboard (created by Cut or Copy) into the design, allowing elements to be re-used in different areas of a design or in other Cut2D Pro parts.

Drawing | Plate Production

This command is for designing and engraving multiple badges or nameplates using variables for positioning imported data from a text file list. The production plate functionality is typically used by engravers making badges from a database file supplied by a customer, but could also be useful for making nameplates for hotel rooms with consecutive numbering.

Procedure

Draw and Setup the Master Template

Create a New job and specify the Material Size to equal the Sheet size the badges will be cut from.

Layout the badge / plate at the required size and using the Text Tools add variables where imported data / text is required. Variables are defined using double exclamation marks ('!!') at the start and end of the variable name.


Calculate Toolpaths

Select and calculate the toolpaths for each of the elements on the design. For example, calculate an engraving toolpath for the text and logos and a separate Profile cut-out toolpath around the outer edge to cut out the design

Use the Plate Production Tool on the master template

With all of the vectors that make up the master template selected, click on the Plate production tool to open the Plate Production Dialog window.

The Plate Production Dialog

The left side of the Plate Production form is used to layout the plates / badges on the selected sheet of material, and shows the total number of plates that can be engraved / machined from each sheet of material.

Material Size

This is the material sheet size that the badges will be engraved onto. If the number and size of the badges requires additional sheets of material to be used the software automatically creates a separate layer for each sheet required.

Plate Size

This is the size of the selected Plate / Badge and is based on the bounding box of the selected vectors.

Sheet Margins

This specifies the border margin between the edge of the material sheet and the plates.

Independent margin spacing can be set for the Top, Bottom, Left and Right sides of the material

Equal Margins ensures the same space is added around all 4 sides of the plates.

Spacing

This is the horizontal and vertical spacing between each Plate / Badge.

Number of Plates

The number of plates that will fit on to the specified material sheet size is automatically calculated. This calculation takes the plate size and adds the Sheet Margins and Plate Spacing to determine the maximum number of plates that can be made from each sheet.

Toolpath Options

If toolpaths have been calculated for the master Template this option is available.

Checking ✓ this option automatically calculates toolpaths for all the plates / badges in the project.

Unchecking this option only creates the vectors for each plate / badge.

Import the Data to be Merged into the Template

The right-hand side of the Plate Production form is used to select the data that will be merged into the template, and how the data will be interpreted to create each plate / badge

Import the required text / data file using and select the appropriate format separator.

The data file is commonly created using a spread sheet such as Windows Excel. Use the option to Save As or Export to obtain the required file format that includes the correct Separator information.

Separator

The separator is the method used in the data file for dividing each set of information into columns. The most commonly used options are: Comma, Tab, Semicolon or a Space

First row is column names

It's very common for the first row of data in a file to simply show what each of the field names are, and this information is not used on the badge or plate. Checking the box First row is column names tells the software to start working with data from row 2

Assign the Variables to the data in the text file

All of the variables specified on the template - text with double exclamation marks '!!' on either side '!!' are automatically listed on the form. These variable names are each assigned to a data field (column of text) inside the data file.

Variable Assignment

Click to select a Variable Name then select the data field from the imported file that is required on each badge / plate i.e. the person's name

Repeat for each of the Variable Names listed on the form

Number Formatting

Variables can be assigned to Text from a data file - Names, Dept., etc. or to a Counter number that can be formatted and incremented using the Number Format options.

Calculate

Click to create all Badges and associated Toolpaths

If toolpaths have previously been calculated for the vectors in the Master Template, the option to automatically Create Toolpaths for each badge / plate is switched on in the bottom left corner of the form.

Close

Click to finish plate production and close the form

Multiple Sheets

Multiple Layers are automatically created if multiple sheets of material are required to engrave all of the badge data from the imported text file. Layer named Sheet 1 is displayed in the 2D view showing the badges on this sheet.

Each of the Sheets is on a different layer and can be set visible or invisible using the Layer Manager.

Multiple Toolpaths

When Toolpaths are automatically calculated, a separate toolpath for each operation on each sheet of material is calculated and named using the convention 'S1 - Name', where the Name is the name of the toolpath previously calculated for the template.

Drawing | Redo Operation

Clicking this option steps forward through design steps that have been Undone using the Undo command (see above) to get back to stage that the user started using the Undo function.

Drawing | Rotate

For precise control of the rotation, or to use a point other than the selection's center as the rotation center, you can open the rotation form from the Drawing Tab.

Selected items in the 2D View can be rotated to a new orientation using this tool. The rotation options form can be activated from the tool icon on the Drawing Tab. Alternatively you can use the interactive transform mode (where the form is not required) directly from the 2D View.

With this form open the additional Pivot Point handle is available (two concentric circles initially positioned at the center of your selection) for you to click and drag in the 2D View. The Pivot Point (around which the selection will be rotated) responds to the currently enabled snapping options to help you to position it precisely on significant locations within your artwork. Hold down the Shift key to temporarily disable snapping while you drag the Pivot Point.

Pivot Point

On the form there are also six radio button options for snapping the rotation Pivot Point to the selection itself or to a precise position. The first five options allow you to snap to the corners and center of your selection.

Use Coordinates

The X and Y edit boxes allows you to precisely specify the position of the Pivot Point. This is also the option that will be selected by default if you drag the pivot point using your mouse directly in the 2D View.

Type of Rotation and Angle

This controls what the angle value does.

  • Relative will simply rotate the object by the given angle. For example, you can enter a small angle, and then rotate multiple times to nudge the object a little bit at a time. A positive angle results in a counter clockwise rotation. A negative angle results in a clockwise rotation.
  • Absolute will set the rotation of the object to the given angle. For example, setting a zero angle here will reset the rotation of the object back to its original orientation (as long as the rotation hasn't been baked).

Keep in mind that when rotating an object, it's rotation is maintained so that you can restore the rotation or scale along its original axes later on if required.

Interactive Rotation

Generally the most convenient way to rotate an object in the 2D View is to use interactive transform. This mode is initiated by clicking the selected object twice with the cursor. The process is:

  • Select the object by clicking on it in the 2D View (or multiply select objects using box selection or by shift-clicking on them).
  • Click the selection a second time to activate the interactive options rotation handles on the selection box.
  • Click and drag on the blue handles (solid squares) at the far corners of the selection to rotate it.

Note

Holding down an Alt key when dragging to rotate the object snaps to angular rotation steps of 15° increments, this incremental value can be edited in the Snap Setting dialog (F4).

Drawing | Save a File

This option opens the File Save As dialog window and allows the job to be saved as a Aspire file. Navigate to the required folder, enter a suitable name for the job and click the Save button.

You can also change the Save As Type using the Dropdown menu. This will allow you to save your file in the .CRV VCarve Pro file type. Saving with this file type will remove all 3D clipart and other 3D Data that is not usable in VCarve Pro, and will allow you to open a file from Aspire in VCarve Pro.

Drawing | Set Size

Selected items in the 2D View can be accurately scaled or resized using this option.

Anchor

The anchor position determines the point on your selected object's bounding box that will be resized to the dimensions entered.

Link XY

Checking ✓ this option will always scale the height and width in proportion. Leaving the Link option unchecked allows non-proportional scaling

Auto Scale Z

This option sets a specific mode of scaling for 3D Components. When it's checked, ✓ scaling a model component in X or Y will result in it also scaling proportionately in Z, as such if you increase its size in X and/or Y then its Z Height will also increase and conversely when you reduce its X and/or Y size it will shrink in height. When it is unchecked then the Z Height of your Components will remain constant regardless of any X and/or Y scaling done either within this form or dynamically using the mouse in the 2D or 3D View.

Interactive Sizing

The default mode is to enable selected items to be scaled interactively by clicking twice with the mouse.
The process is:

  • Select the vectors
  • Click a second time to activate the interactive options - handles on the selection box
  • Click and drag on the white handles

The keyboard shortcut T opens the Scale form in interactive mode

Drawing | Snapping Options Dialog

To help with drawing, construction and layout, the 2D View has Rulers which are displayed along the top and down the left side of the window. In addition to the Rulers there is the option to use Guidelines and The Smart Cursor to help with construction of vectors or positioning of other objects in the 2D View.

Rulers

  1. The Rulers are permanently displayed in the 2D view to help with positioning, sizing and alignment. The graduated scale automatically uses the units set for the project and zooming in / out shows the sizes in 10ths.

Guidelines

Guide Lines are used to help layout designs and make it very easy to sketch shapes by clicking on the intersections of Guides. Guide Lines are easily be added to the 2D view by pressing the left mouse button down on the appropriate ruler (left if you want a vertical guide and top if you want a horizontal guide) then holding the button down and dragging the mouse into the 2D view.

While dragging a Guide into position it automatically Snaps to the units displayed on the ruler. This snapping behavior can be overridden by holding down a Shift key while dragging the guide. After positioning a Guide it can easily be moved to a new position by clicking the right mouse button on the guide to open the Guide Properties form as shown later in this section. If you hover the mouse over a Guideline then its current position is displayed next to the cursor

Additional guide lines can be added relative to an existing guide line by interactively placing the cursor over an existing guide (the cursor changes to 2 horizontal arrows), Holding a Ctrl key and dragging to the required position. The incremental distance between the guide lines is displayed next to the cursor. Releasing a Ctrl key changes to display the absolute distance from the material origin.

Guides can also be added and other edits made by right clicking on the Guideline which will bring up the Guide Properties form:

The exact position can be specified by entering a New Position.

Guides can be given an angle by either entering an angle into the New Angle box or dragging the slider and clicking . Angles are measured in degrees counterclockwise from the x-axis. From an angled guide you can only create relative parallel guides.

Guide lines can be locked in position to stop them from being inadvertently moved by ticking the Lock Guide option.

Additional Guide Lines can be added that are positioned using absolute or incremental coordinates. Enter the Absolute or relative positions and Click .

Guides can quickly be toggled visible / invisible by clicking in the Top Left Corner of the 2D view:

Alternatively the visibility can be changed using View Menu ► Guide Lines from the Main MenuView Menu ► Guide Lines ► Delete All Guides from the Main Menu

Snapping Options

These options can be used to help create and edit vector geometry.

The Snapping Options form can be accessed by selecting Edit ► Snap Options from the Main MenuF4.

Display Text at Cursor

Displays the XY coordinates on the cursor making it easy to see the position for each point

Snap to Guides

When this option is checked ✓ drawing and positioning vectors will snap onto any horizontal or vertical guide lines visible in the 2D view.

Snap Guides to Geometry

When checked, ✓ the Guide Lines can snap to Geometry while being dragged.

Snap to Grid

Displays a grid of points separated by the Grid Spacing which can be snapped to when drawing or editing vectors and other objects in the 2D View.

Snap Distances

Snap to fixed lengths based on your zoom level. This occurs when creating shapes, dragging nodes or vectors.

Snap to Job Center and Corners

Snap to the job corners and center. This, also, control the job smart snapping

Fixed Nudge Distance

Objects can be moved small, fixed distances (nudged) by holding Ctrl + Shift and tapping the arrow keys. The Fixed Nudge Distance specifies the distance to move selected objects with each nudge.

Snapping Radius

The snap radius (pixels) will adjust how close the cursor must get to vector geometry in order to snap it. If you work quickly and grab and throw geometry at speed, you may prefer a larger Snapping Radius to pick up geometry that is vaguely near the mouse. If you work precisely or have complex overlapping geometry, you may prefer a smaller Snapping Radius to avoid having to zoom in to select one geometry in an area that has many nearby vectors.

Geometry Snapping

Used to control the position at which the cursor will snap when drawing and moving objects. When drawing, the cursor will snap to items on vector geometry depending what options you have selected in the form under this section.

Object centers, Span End points, Span Mid-points, Arc centers, intersections Horizontally, Vertically and the specified Angle and Distance Guide lines and the intersection of Guides

Snap to Nodes, mid-points, centers
Snap to Nodes, mid-points, centers
Snap to Guides, matching horizontal and vertical points, plus angle and distance
Snap to Guides, matching horizontal and vertical points, plus angle and distance

Smart Snapping

Smart snapping works by snapping the cursor to imaginary lines related to vectors and/or nodes. These lines will appear as dashed, and sometimes coloured, lines that go through the vector or node and the cursor point. You can snap to the intersection of those lines by hovering over the nodes that you're interested in. This reduces the need to create construction geometry (for example, for aligning nodes or vectors), and can be used in almost all the shape creation tools, node editing and transforming vectors.

Note

A node is the start, middle, or end point of a span.

Note

The snapping system is watching to see which vectors you hover the mouse over. It remembers that last few vectors as the ones you want to work with and draws the snap lines for those as a priority. There is a maximum number of nodes and vectors that can be "woken up" at the same time to avoid too many snap lines appearing at once.

Snapping lines can be drawn from:

  • Nodes that were woken up by hovering the mouse over them or their span
  • Vector properties, such as their bounding box or center point
  • Material properties, such as extensions from the edge and the middle

Note

It is possible to wake up vectors on the other side of a double-sided job.

Cursor

Type

Description

Object Bounds

The theoretical bounding box surrounding the active vector
+ horizontal and vertical lines passing through the centre

Horizontal and Vertical Lines

Horizontal and vertical lines passing through a node or a span midpoint.

Tangents

Tangents originating from a node or a span midpoint.

Perpendicular to Tangents

Lines which are perpendicular to tangents from nodes or span midpoints.

Connecting Lines

Lines connecting two nodes. Includes mid-point.

Span Geometry

Snap to the geometry of the vector.

Angular Constraints

Snapping to specific angles, as defined in the snap options F4.

Job

Horizontal and vertical lines through the center of the job.

Object Bounds

These snap lines appear on the bounding box edges of the vector, and in the middle horizontally and vertically.

Bounding Box
Bounding Box
Object Center
Object Center

Vertical and Horizontal Lines

Nodes

The snap lines appear when the cursor is near the horizontal or vertical line passing through the woken nodes.

Vectors

Snap lines become available while moving vectors so that it is used for aligning them with other vectors.

Vertical
Vertical
Horizontal
Horizontal

Tangents

These snap lines originate from the woken node and will appear as an extension along the end of the belonging span.

[object Object]
Tangent

Perpendicular to Tangents

These snap lines will be 90° from the tangent snap line.

[object Object]
Perpendicular

Connecting Lines

If you wake two or more nodes, you could snap to the line connecting them. You could, also, snap to the mid-point of that line.

[object Object]
Connecting Lines

Span Geometry

This allows you to snap to the geometry of the vectors.

[object Object]
Span geometry

Angular Constraints

[object Object]
Angular Constraints eg. 30° (Angle step 15°)

Job Edges & Centre

If you have the job snapping

[object Object]
Job Center

Toolbar Snapping Options

Geometry Snapping, Smart Snapping and Grid Snapping can be switched on and off from the View Toolbar

Any change to the snap settings F4, through the Main Menu or the toggles on View Toolbar will be remembered for subsequent sessions.

Disable snapping temporarily

Snapping can be temporarily disabled by holding down the Shift key.

Drawing | Subtract Vectors

Selected closed vectors that overlap can be merged together to create a new shape. These tools consider the closed vectors to be solid areas.

The following examples begin with these five vector shapes where the rectangle was selected last.

Areas in the first shapes that overlap the last selected shape are removed. In this case, the last selected shape was the rectangle, so the rectangle is cut away from the circles anywhere that overlaps.

Drawing | Text On A Curve

This tool requires the user to select a single line of text with the Draw Text tool and a single vector curve/line. It will take the text and fit it onto the selected vector to follow the curvature. Options within the tool allow position, space and location against the line to be edited.

To edit properties of text object that was already on a curve, just select the text object. To place it on another curve select both the text object and a vector.

It is also possible to use a closed vector to wrap the text around it.

Text Size

Maintain text Size

Will not change the size of the text block

Scale text to fill curve

Will increase the character size in order to fit along the entire length of the selected curve.

Text Spacing

The slider can be used to increase or decrease the word and character spacing. Each time the form is opened, or new text is selected, this control starts at the 100% mark. While this text is being edited the spacing scale can be increased or decreased from its original value.

Text Position

Above Curve

On Curve

Below Curve

Text on other side

Offset Distance

Allows the text to be moved away from the curve by a specified distance.

Text Alignment

The 3 options allow the text fitted to the curve to be aligned to the left, middle or right hand side of the selected curve. Or, when using a closed vector curve, relative to the Start Node.

Note

Remember the Start node can be changed using the Node Editing Tools available from the Right mouse menu and selecting Reverse Direction.

Characters in the text string can also be aligned 'normal' to the drive curve or left in the original vertical position.

Align to Curve
Align to Curve
Keep Vertical
Keep Vertical

Position on the curve

The text's position on the curve can be adjusted interactively, by dragging the anchor point handle in 2D View.

[object Object]
Dragging text on a curve

Detaching from the curve

The text object that was wrapped on a curve can be detached from it.

To detach text right-click on the selected text object and select "Remove Text From The Curve" option.

Drawing | Text Selection

The Text Selection tool allows the user to adjust kerning, line spacing and bending the text on an arc. The text will be displayed as magenta lines with 2 Green handles in the middle for arching the text.

[object Object]

If the selected text was placed on a curve the handles will not appear, as such text cannot be arched.

Letter Kerning

The interactive kerning and line spacing cursor is shown when placed between letters or lines:

[object Object]

The interactive letter kerning allows default text to be modified so that adjacent pairs of letters sit more naturally together. A typical example is shown above where the capital letters W A V are placed next to each other and the default space is excessive.

Place the cursor between 2 letters and click the Left mouse button to close the gap.

Holding a Shift key and clicking the Left mouse button moves the characters apart.

Holding a Ctrl key when kerning doubles the distance each letter moves on each click.

Holding Shift and Ctrl keys together and clicking the Left mouse button moves the letters closer together in larger increments.

Line Spacing

Line spacing can be modified by placing the Edit Text cursor between lines. It will change to the line spacing cursor:

[object Object]

Clicking Left mouse button will move the adjacent lines of text closer together.

Holding the Shift key and clicking the Left mouse button will move the lines apart.

Holding the Ctrl key doubles the distance each line moves on each mouse click.

Holding the Shift and Ctrl keys together and clicking the Left mouse button moves the lines apart in larger increments.

Text Arching

The interactive rotation and movement cursor is displayed when the cursor is placed over either of the Green Handles to indicate that the text can be arced either Upwards or Downwards:

Bend Text Upwards
Bend Text Upwards
Bend Text Downwards
Bend Text Downwards

Click and Drag the Bottom Green box to arc the text Downwards.

Click and Drag the Top Green box to arc the text Upwards.

The text can easily be dragged back into the horizontal position again.

After arcing text, additional Red and Blue handles are displayed for Rotating and Moving the text.

[object Object]

Moving

There are two white handles for moving the text, one in the middle of the text, and one in the center of the arc, though that may be off-screen for very shallow arcs.

Rotating

Clicking and dragging the Red boxes rotates the text around the center point of the arc.

Holding the Ctrl key forces the rotation to be in 15° increments. This allows the text to be positioned exactly on the horizontal or vertical quadrants, even after it may have been moved slightly.

Changing arc radius

Clicking and dragging the Blue boxes changes the radius without moving the arc center.

Drawing | Trace Bitmap

This tool automatically traces or fits vectors to image files so they can be machined. Use the Import Bitmap tool and select the image in the 2D view, then open Fit Vectors to Bitmap.

After importing an image the Tracing option allows vector boundaries to be created automatically around colored or black and white regions in the image.

Tracing a Selected Area of the Bitmap

You can define an area within the bitmap, such that only that part of the bitmap will be traced. This can be done by selecting the bitmap (if this hasn't been done already), and then clicking and dragging the mouse over the area you want, to define a rectangular region on the bitmap. This will be highlighted with a dashed black rectangle.

Clicking on the Bitmap again will remove a selected area if one has been specified, in which case, the entire bitmap will have vectors fitted to it.

Tracing Black and White Images

When working with Black and White images the slider can be used to change the Threshold and merge the levels of gray between all white (min), and all black (max).

When the image being displayed in the 2D view looks correct then clicking the button automatically creates vector boundaries either around the selected Trace Color or the grayscale.

Tracing Color Images

Color images are automatically reduced to 16 colors and the slider allows the visible number of colors to be set as required. Colors are merged with the closest match.

Colors can be temporarily linked together by clicking the check boxes next to each of the colors displayed. This changes the color displayed in the 2D view to the selected Trace Color. This is very useful for merging similar color's together to allow complete regions to be traced.

If a new Trace Color is selected the linked colors are displayed using this color in the 2D view.

The Reset button unlinks all the checked ✓ colors and the image displayed in the 2D view reverts back to the original 16 color image.

Tracing a Selected Area of the Bitmap

You can define an area within the bitmap, such that only that part of the bitmap will be traced. This can be done by selecting the bitmap (if this hasn't been done already), and then clicking and dragging the mouse over the area you want, to define a rectangular region on the bitmap. This will be highlighted with a dashed black rectangle.

Clicking on the Bitmap again will remove a selected area if one has been specified, in which case, the entire bitmap will have vectors fitted to it.

Fitting-Options

The options available on this form control how closely the vectors fit / follow the selected color boundaries and these can be modified to obtain improved results.

Corner Fit

The Corner Fit control determines how accurately the vectors are fitted to the corner edges in an image.

Loose
Loose
Tight
Tight

Noise Filter

The Noise Filter slider controls the minimum size of pixels that are traced / vectorized, preventing small unwanted vectors or noise being created.

Bitmap Fading

Preview

This will preview the result of the tracing of the bitmap. If you are not happy with the result provided, you can alter the settings and click on the button again to get an updated result.

Apply

When you are happy with the result of the preview you can click on the button to keep it.

Drawing | Trim Objects

The trim tool allows you to trim all the objects inside a given boundary. It is much more efficient than manually trimming all the contours with the trimming scissors, and allows the trimming of closed contours, open contours and components.

To use:

  • Select objects you wish to be trimmed
  • Select the object you wish to trim against (hold shift to add to selection)
  • Choose to clear inside or outside

If the Clear outside boundary option is selected then all the objects that intersect this boundary are clipped, and the area outside is removed. If the Clear inside boundary option is selected, then the parts of the selected objects which lie inside the boundary are removed.

Geometry before trimming. Select the lines first and then the circle
Geometry before trimming. Select the lines first and then the circle
Trimmed vectors using Clear inside boundary
Trimmed vectors using Clear inside boundary
Trimmed vectors using clear outside boundary
Trimmed vectors using clear outside boundary

If you want to use multiple vectors for the trimming boundary, they must be grouped for trimming. To group a collection of vectors select the vectors, right click and choose Group Objects from the drop down menu, alternatively select all the vectors and press the G key.

Trimming with Group

Drawing | Undo Operation

Clicking this option steps backwards through the design changes made by the user.

Drawing | Ungroup Selection

Ungroup a set of Grouped vectors back to its individual vectors before it was grouped.
The Shortcut key for this operation is U.

Ungroup to the group's layer

By default, when grouped objects are ungrouped they revert to the layers on which they had previously been located before the grouping operation. However this is sometimes inconvenient. For example, when you have copied a group of vectors to a new layer, it is easier for subsequent editing if the copied vectors to remain on the new layer, even after ungrouping. An alternative right-click pop-up menu command has been added to make this process easier.

A shortcut key combination is also available to provide support for both of the ungroup operations. In summary, therefore, the group and ungroup shortcut options are as follows:

  • G Group the selected objects
  • U Ungroup the selected objects to their original layers, sub-groups remain grouped.
  • Ctrl + U Ungroup the selected objects to the group's layer, sub-groups remain grouped.
  • Shift + U 'Deep' ungroup the selected objects to their original layers. Sub-groups are also ungrouped.
  • Ctrl + Shift + U 'Deep' ungroup the selected objects to the group's layer. Sub-groups are also ungrouped.

Drawing | Vector Boundary

The Vector Boundary form allows you to create boundaries around selected vectors.

Offset Boundary

When this is checked ✓ the created boundary is offset outwards by the distance specified.

Rubber Band Boundary

When this is checked ✓ the created boundary is the result of stretching a rubber band around the currently selected vectors.

The images below demonstrate the difference between the two types of boundary that the form creates. The picture on the left illustrates the standard offset output and the one on the right shows the result when Rubber band boundary option is checked ✓.

Offset Boundary only
Offset Boundary only
Offset Boundary and Rubber Band together
Offset Boundary and Rubber Band together


Drawing | Vector Selection Mode

When the Vector Selection Tool is chosen, the selected vectors are shown as dotted magenta lines. Vectors need to be selected before any of the editing tools such as scaling and moving etc. can be used.

Vector selection methods

Multiple vectors can be selected in the following ways:

  1. Manual multiple selection:
    Hold down the Shift key while clicking the Left mouse button on each vector required. Objects can be deselected by simply clicking on the object again with a Shift key pressed.
  2. Moving the cursor from Left to Right selects only fully enclosed objects:
    Click and drag the left mouse button moving from Left to Right selects all objects completely inside the selection rectangle.
  3. Moving the cursor from Right to Left selects all objects inside or touching the selection rectangle:
    Click and drag the left mouse button moving from Right to Left selects all objects inside the selection rectangle + any that the selection touches.
  4. Pressing the keyboard keys Ctrl+A will select all vector objects in the design:
    Selected vectors are displayed as dotted magenta lines.

Deselecting Vectors

Selections can be cancelled by:

  • Left clicking on an area outside the selection
  • Pressing the Esc key
  • Pressing the Right mouse button and clicking Selection ► Unselect All from the pop-up menu.
    You must click on the white drawing background to get this option in the pop-up menu.

Drawing | Vector Texture

Repeating texture patterns can be created using the Create Vector Texture tool. These vectors can be machined in a variety of ways to create attractive textures.

To use the tool click the icon on the drawing tab. If required, select any contours that you wish the pattern to be created within. By using the sliders and edit boxes on the form the style of the created pattern can be varied. Click Preview to see a preview your created texture as you adjust the form's parameters. When you are happy with the preview, click OK to create the pattern.

Angle

The lines in the texture are created at an angle. This value can be set to any value between -90 degrees and 90 degree.


[object Object]
Angle of 30°

Line Spacing

The line spacing controls the distance between the contours created by the tool. Use the edit box labeled Max. Spacing to enter a maximum value of line spacing. The slider underneath the edit box controls the degree of variation in the line spacing. If the slider is to the far left then this mean variation is at a minimum and so the lines are evenly spaced. If the slider is to the far right the variation is highest and so the distance between created contours varies between zero and the maximum spacing specified.

Minimum variation
Minimum variation
Maximum Variation
Maximum Variation

Wave Parameters

Within this section of the form the created pattern can be made to behave in a wave-like fashion. This wave is controlled by two parameters: the amplitude and wavelength.

Wavelength

The wavelength describes the length over which the contours shape repeats itself. A bigger wavelength gives a long wave while a small wavelength gives a short wave.

Short wavelength
Short wavelength
Long wavelength
Long wavelength

Amplitude

The amplitude describes the height of the wave. Larger amplitude means a taller wave and smaller amplitude means a shallow wave.

Small amplitude
Small amplitude
Large Amplitude
Large Amplitude

Noise

The noise slider controls the degree of randomness applied to the above values and can be used to create less regular patterns.

No noise
No noise
Medium noise
Medium noise
High noise
High noise

Vector Layer

To create the vectors on a new layer make sure the check box labeled Place Vectors on Layer is checked ✓ and enter the layer name into the edit box labeled Name.

Drawing | Vector Unwrapper

This tool converts a vector into another vector suitable for using with the two-rail sweep tool to create rotary models from a desired cross section.

To unwrap the vector, to the following:

  1. Select the contour you wish to unwrap
  2. Use the options or the drag handle to select the center of the unwrapping
  3. Press

The contour generated can now be used with the two rail sweep tool to create rotary models.

Note

This tool is only available in rotary projects.

[object Object]
Vector before unwrapping. The drag handle and a circle demonstrating the diameter of the model are shown.
[object Object]
Vector after unwrapping

Center of Rotation

The center of rotation for the unwrapping changes the unwrapping of the contour so that when the resulting contour is used to create a rotary model, the center of rotation of the model is the chosen point.

Use center of contour

Sets the center of rotation to be the center of the bounding box of the selected contour

Use center of workspace

Sets the center of rotation to be the center of the workspace.

Use custom point

Sets the center of the job to be a specified point. The custom point can also be chosen by selecting the drag handle and dragging to the desired point.

[object Object]
Drag Handle

Refine unwrapped vectors

Typically the resulting unwrapped contour will contain a large number of nodes. Selecting this option will result in an unwrapped contour with far fewer nodes.

Drawing | Vector Validator

The Vector Validator is intended to help find issues with contours after file imports that are stopping tool-path creation such as overlapping contours or intersections. It also indicates zero-length spans.

The Vector Validator dialog can be opened with a selection to work on. If there is no selection, all visible vectors on the current Side of the current Sheet on visible layers will be validated. The selection can be changed while the form is open.

The text on the button changes to show whether all vectors or just the selection are going to be searched. While searching, the Search button becomes a Stop button.

To cancel a search, click the or button.

Issues found so far will be marked.

Marks

Examples of the marks described on the form are shown below:

If zero-length spans are found, the button is enabled. Clicking this will remove the zero-length spans and clear their markers

V-Carving Mode

When this is checked, the Vector Validator will perform its checks on vectors as it is performed and necessary for V-Carving.

For example,

  • It will ignore intersections that may exist within text as it may be because of issues in the font. If you get intersections involving the text, then you could try to weld it and run the Vector Validator on the result.

Drawing | Weld Vectors

Selected closed vectors that overlap can be merged together to create a new shape. These tools consider the closed vectors to be solid areas.

The following examples begin with these five vector shapes where the rectangle was selected last.

Welds overlapping vectors together to create a new shape which follows the outermost edge of all the selected shapes.

When welding text, the internal regions of characters are preserved.

Overlapping text before welding
Overlapping text before welding
Overlaps removed by welding, but internal regions preserved
Overlaps removed by welding, but internal regions preserved

Layers | Layer Management

Vectors and Bitmaps can be assigned to different layers.

All the objects assigned to a layer can then be simultaneously selected, labeled, colored, temporarily hidden or even locked (to prevent accidental editing) using the Layer Management tools. Even for relatively simple designs, organizing the elements of your artwork onto layers can make managing your project much easier.

Managing Layers

You can access the tools needed to manage layers from two locations: the Layer Control on the View Tool Bar, and the Layer List on the Layers tab.

The Layer Control on the View Toolbar

A Quick Access Layer Control is conveniently located above the Views in the View Toolbar. This tool provides a pop-up Layer List, from which you can quickly change the selection of the active layer, add a new layer, or modify the properties of any existing layer. When you have finished, click anywhere outside of the Layer List window and it will cause it to close.

The Layers Tab

To get a complete overview of the current layer structure of your artwork while you are working, or to carry out more extensive organization of the layers, you can also use the Layers tab. The Layer List is identical in both the Layer Control and the Layers tab, but the latter can control layer ordering and be left visible, pinned or even undocked, while you continue to work on the artwork itself

List Item Command and Icons

Each layer in the list has five elements:

Status Icon

[object Object]
Status Icon

The leftmost icon indicates whether the layer is currently visible or hidden. Click on this icon to toggle the visibility of the layer.

The presence of a padlock shows that the layer is locked and cannot be accidentally edited.
Right-click the layer in the list and select the Unlock command to alter this.

Layer Colour

[object Object]
Layer Colour

The color swatch can be used to color all the vectors on a layer. Click on the swatch icon Layer Color Icon and select a pre-set color from the color selector dialog, or choose to create an entirely custom color.

Layer Content

[object Object]
Layer Content

The layer content icon will be grayed-out as an additional indicator that the layer is not currently visible. Layer Empty Content Icon a blank white sheet indicates that the layer does not currently contain any objects or vector geometry. If you import files from 3rd party CAD drawing packages via DXF or DWG format it is common for the file to include empty layers. This icon allows you to identify these empty layers and delete them.

Layer Name

To change the name of a layer, you can double click on this part of the layer item in the list to trigger in-situ editing. This works in the same way as file renaming in Windows Explorer. Alternatively you can right-click or use the layer's Pop-Up Menu icon to select the Rename command.

Pop-up Menu

[object Object]
Pop-up Menu

Click the pop-up menu icon Pop-up Menu Icon for access to Activate, Lock, Insert, Delete and Merge layers as well as further ways to choose which layers to show and hide.

Select All on a Layer

Double-clicking on a layer in the Layers List will select all the objects on that layer. Alternatively you can choose the Select Layer Vectors command from the layer's pop-up menu.

Layer Ordering Arrows

Adjacent to the Layers List heading label are two arrow buttons. These move the selected layer up or down in the Layers List. This can be important to set the drawing order of objects that might otherwise obscure one another (specifically Bitmaps and 2D Component Previews). Objects on the top layers in the list are always drawn before objects in the lower layers and will, therefore, be 'underneath' them in the 2D View. You can use the Layer Ordering Arrows to resolve this issue.

Add New Layer

New Layers can be added using the Add New Layer button. Alternatively a new layer can be created directly from the 2D View by right-clicking an object and selecting either the Copy to Layer ► New Layer... or Move to Layer ► New Layer...

Layer Name

It is always preferable to take the opportunity at this stage to give your new layer a meaningful name relating to its content or purpose. Later on this name will make it easier for you to manage your layers as your design becomes more complicated

Drawing Color

All the vectors on this layer will be colored according to this setting. This can be a very useful way of distinguishing between the vectors that are on different layers, directly in the 2D View.

New Layer is Visible

With this option checked, ✓ the new layer will automatically be visible as soon as it is created.

New Layer is Active

With this option checked, ✓ the new layer will automatically become the active layer and any subsequent vector creation or manipulation will occur on this new layer.

Insert New Layer

An even quicker way to add new layers is via the Insert Layer command from a layer's right-click Pop-Up Menu. This command will create a new layer above the selected layer which will be visible, unlocked and colored black. After creation the new layer item's name is ready to be immediately edited by typing a new name in.

Moving Objects to Layers

Objects on any layer can be moved onto another layer by right-clicking the object in the 2D View and selecting Move to Layer from the pop-up menu. It is also possible to place a copy of selected object to another layer by selecting Copy to Layer from the pop-up menu.

Clipart | Clipart Tab

The Clipart tab provides quick and convenient access to V3M files or 2D vector artwork.

This tab includes the library browser that allows you to add folders containing V3M Files into the software or you can use the local files option that allows you to quickly see the contents of several folders of V3M files in one place.

Importing Clipart

To import a file as a piece of clipart you can simply double click its thumbnail to position the clipart in the center of the job. You could also Right click on a piece of clip art and choose the option, this has a sub-menu that allows you to choose an existing Level or to create a New Level. When creating a New Level you will be prompted to enter a name and choose a combine mode. You can also click on a preview image and 'drag and drop' its thumbnail from the clipart browser, into the 2D or 3D View. To do this:

  • Move your mouse over thumbnail image in the clipart browser.
  • Press and hold down the left mouse button.
  • While holding down the left mouse button, move the mouse back into the 2D or 3D View.
  • A copy of the thumbnail image will be 'dragged' with the mouse pointer.
  • Release the mouse button to 'drop' the clipart file into the 2D or 3D View.

The selected component clipart model or vector outline will be imported at the location of the dropped thumbnail and, if appropriate, added to your model's Component Tree

Library Browser

The library browser provides quicker access to folders on your computer which are in frequent use, or perhaps hold the data for the current project you are working on.

To add a folder into your library click on the button which opens up a dialog asking you to choose the folder you would like to add. Navigate through the tree to choose then folder and click OK. Unlike the Local Files browser the Library browser will only show the clipart that within this folder and folders within this folder. You will not be able to see the whole of the file tree beneath this folder.

Once you have populated your library with folders then clicking on a folder will populate the clipart browser with the objects which are contained in this folder and show you any subfolders immediately below it.

To better understand this, consider the following example: My current project is a western saloon themed sign. I have split up all the resources I am using for this creation into three folders, so that I have the following file folder structure:

Removing Folders

To remove a folder, select from the list of folders and click on the button. This will not delete clipart from your computer; it will just remove the library folder

Adding Folders

Folders may be added to the library from the local file browser by right clicking and selecting the Add folder to library option.

Local Files

The local files browser allows you to select a folder using the file explorer tree in the top section of the page. When you select a folder containing Vectric files (*.crv or *.v3m) the bottom section of the page will fill with thumbnail images of the V3M or CRV files within each folder.

Integrated Windows Explorer Thumbnail Support

V3M files automatically include thumbnails. Windows Explorer can make use of these thumbnails to show you a preview of each file when you browse a folder.

Drag and Drop

Aspire supports Windows drag and drop functionality to quickly add V3Ms into an existing model directly from Windows Explorer.

With Windows Explorer and Aspire both open, simply click and drag the V3M thumbnail of the file you want from the Explorer Window into either the 2D or 3D View window of Aspire. The selected V3M file will be imported automatically and added to the Component Tree

Modeling | Add Draft to Model

For some applications it can be useful to eliminate vertical walls on 3D models, especially if the machined part is intended to be used as the basis for a mold or vacuum forming tool.

The Add Draft tool will automatically add a minimum angle to any steep walls that exist in your model. The draft angle is specified by using the slider or entering a typed value in the form.

When the button is pressed, the tool creates a new 3D Component by baking the visible Components and applying the draft angle across all the walls of the composite model. Note that you do not select the Component/s to apply the draft angle to, just ensure that they are visible in the 3D view. The resulting Component will not have any wall angles that are steeper than the specified draft angle. Once complete, both the original Component/s and the new Component will be visible, although the original may be obscured by the new Component. The Component with the draft angle will be named appropriately indicating the amount of draft that was added. The images below show how a Component looks before and after adding 20° of draft.

Original Model
Original Model
With Draft Added
With Draft Added

Note

If you are creating a model within a two sided environment the draft will only be applied to the side you are currently working on. To apply a draft to both sides you will need to switch over to the opposite side and apply a draft to the model there.

Modeling | Baking Components

In general, the most useful feature of individual Components is that they can be manipulated entirely independently of each other to build up simpler design elements into a sophisticated 3D model. There are some editing functions that require the individual element to be consolidated into a single object. For example you may wish to smooth one shape into another using the sculpting tools or bend a group of Components around a curve using the distortion tool. In Aspire, consolidating a selection of Components into a single, new object is a process called 'Baking'. Once baked, the selected Components will become a single Component object and you will no longer be able to access the individual elements.

Cut2D Pro will prompt you when you have a group or Component selection that requires baking before a particular modeling tool or operation can proceed. Alternatively, you can use the Bake command to perform this operation yourself. By manually baking-in existing fade, tilt or distortion, for example, you are then free to apply further dynamic properties 'on top of' the previously applied ones. In addition, consolidating multiple Components towards the end of the design process allows your computer to recover system resources and may give it a welcome performance boost - particularly if you have been modeling using a large number of high resolution or complex Components.

Copy

If you hold the Ctrl key down when you hit the Baking icon it will retain a copy of the original Components and create a new baked Component instead of replacing the original selection.

Modeling | Clearing or Splitting Components

The options to clear areas of a 3D Component, inside and outside of vectors or to slit a vector into multiple pieces are very useful modeling tools. There are many occasions where the standard modeling options may not allow you to create or control the exact shape that you need. Often you may need to create the general shape then crop (cookie cut) the resulting Component either to leave just the part of the shape you want or to make a hole in it. Many examples of this will be covered in the video tutorials supplied with the software.

Original Vectors
Selected Vectors with 2 Rail Sweep
Resultant Cropped component

In the image above and left you can see the vectors selected for a 2 Rail Sweep to make a simple flowing shape. The result of this sweep is shown in the middle image. Our actual leaf edge vector can be seen in the left hand image after cropping the swept shape back to the leaf outline vector.

To use the cropping function you need to select the Component or Components you want to edit first and then select the object last that you want to use as the cropping region. If multiple Components, or a Component group, are selected for this tool, Aspire will prompt for you to bake the Components before continuing. See Baking Component for more information.

Modeling | Component Properties

The Component Properties form allows you to adjust a number of dynamic properties for a selected Component or Level. Adjusting these properties does not make permanent changes to your Components and can be further edited or reset any time until the component is Baked, in which cases they will be made permanent in the Component shape and this form will be reset.

Note

You can only edit the Name, Combine Mode, Base Height and Appearance for the Properties of a Level.

Multiple Selections

If you have more than one component selected while using the Component Properties tool, Cut2D Pro will apply the changes to all the selected components. Some properties where this would be inappropriate (such as the component's name) are grayed-out when there is more than one component selected. These properties must be applied to components one at a time.

Combine with other components

The Combine Mode dictates how the components (or Level) are combined with the objects below them in the Component Tree. This is done by the software starting at the bottom of the list and working upwards. The first level and first component's combine mode determines only how it combines with the modeling plane. The second and subsequent components are combined with the result of everything below them based on their Combine Mode as detailed below. See Component Tree for more details.

Add

Adds the selected component/s to the result of all the previous components in the list.

Subtract

Subtracts the selected component/s from the result of all the previous components in the list.

Merge

Where they overlap, this Merges the selected component/s into the result of all the previous Components in the list keeping the highest part of the overlapping area. This means the higher part of each shape will be what remains in this area.

Low

Where they overlap, this Merges the selected component/s into the result of all the previous Components in the list keeping the lowest part of the overlapping area. This means the lower part of each shape will be what remains in this area.

Multiply

Where there is an overlap, this Multiplies the result of all the previous components in the list by the heights in this component.

Shape Height

Use the slider or type in a specific percentage to scale the height of the selected Component(s) up or down based on its current height (100%).

Enter a value in the Shape Height edit box directly, or use the slider to adjust the height of your component selection interactively. In either case, the 3D view of the component will update automatically as you adjust the value. The range of available heights on the slider is determined by your current material thickness setting. If these values appear to be inappropriate you can still enter any value you like into the associated edit box, or you can close the tool and select Edit ► Job Size and Position from the main menu. In the Job Setup page you can then correct the current setting for the material thickness before continuing.

Base Height

Enter a specific value into this box to raise the Component or Level up on a flat plane of the thickness you specify. This can be useful to help move an object up so it sits proud of another component it is Merging with. If you are not sure of the value you need, then enter an amount and hit the space bar to apply this. If this is not correct, type in another value and hit space again to apply the new value, look at the 3D View to judge the result - repeat until you get the value you need.

You can also apply a Base Height to a Level. Adding a base height to a level will add the same base height visually to the components in that Level, however the components themselves will have no base height added to them within their properties. This is useful to raise a set of objects on a Level above things that need to appear to be behind them (for example above a textured area).

Note

Level Base Heights are not included in Baking operations on the Components on those Levels but are a separate value that is added on after the objects on the Level have been combined. They are scaled proportionately though when the Scale z height of Model function is used to adjust the Z Height of the Composite Model (visible components).

Reset Heights

The button will remove the dynamically applied Shape and Base height settings from the selected component. To reset the Base Height back to zero using the slider control, double click the central line marker above the slider bar.

Fade

When this option is checked ✓ the user can fade the Z depth of the Component. The first part of this operation (once the option is checked ✓) is to select the button - then click two points in the 2D view. The first click specifies the point which will remain at the current height. The second click specifies the point that the Component will be faded down toward. The shape will fade down from the first point to the second by the percentage selected. Change the strength of the fade by clicking the down arrow next to the percentage value and using the slider to move this up and down or type in a specific value for the amount you would like to reduce the depth by. The fade will be applied linearly between the two selected points. This is a useful tool for giving the effect of a Component fading into the distance to help with overlapping areas of Components if you want to lower an area to give it the appearance of going behind another one.

Tilt

When this option is checked, ✓ the user can set a direction and angle to tilt the Component up in the Z axis. The first part of this operation (once the option is checked ✓) is to select the button - then click two points in the 2D view. The first click specifies the point which will not move (the pivot point of the tilt). The second click specifies the point that will be tilted upwards by the specified angle (the point that will be raised up). Change the tilt angle by clicking the down arrow next to the value, you can use the slider to alter this, or type in a specific value for the angle. This is an extremely useful function for raising a part of one Component above another one when they overlap, without having to raise the whole Component up using the Base Z Position option. In some cases this allows the overlapping areas to sit proud without having to create a deep raised wall around the whole edge of the Component.

Bake

Sometimes it's useful to apply a component's dynamic properties permanently, one example where this is useful is so that further dynamic changes can be applied 'on top' of previous ones. To do this, use the button.

Appearance

Cut2D Pro gives you a lot of control over the appearance of the 3D shaded image for visualization purposes, such as customer approval proofs or marketing material. Each component can be given an individual color or material.

Same as Parent

Use appearance of the objects parent. This is a level for components and the model in case of level. This will ultimately use the model's appearance, as specified in Job Setup.

Solid Color

This option allows to use a single color for shading the component.

Use Material

When this is selected the user can choose from the list of pre-defined material effects by clicking on the box immediately below the Appearance choice. These include many wood grains, metal effects, stone and plastic.

Additional materials can be added to the library. See Preview Toolpaths for more details.

Color from Children

This option is used for a Group of Components or Level and will allow the software to use the individual colors and materials assigned to the groups constituent Components to display in the shaded image even though it is a Group. If this option is not selected the Group/Level will be given its selected Color or Material.

Highlight Selected Component

When choosing a material or color to use for a particular component, the red selection highlighting of the component can prevent you from seeing your chosen material accurately in the 3D view. You can un-check this box to temporarily disable the red highlighting while you make your selections. This option will automatically be re-enabled on exiting the Component Properties page.

Close

The button will exit the Component Properties form and return to the standard set of modeling icons.

Modeling | Component Tree

The model that you see in the 3D View is the result of progressively combining all of the visible components from the bottom of the Component Tree, to the top. The resulting model is known as the Composite Model. The order in which components are combined can have a significant impact on the final shape of the composite model and so you will often need to move components relative to one another within the Component Tree in order to achieve the end result you are intending.

For more information, see the 3D Design and Management page.

Combine Modes

To help you understand how the components are being combined, each component in the tree has an icon indicating how it is currently being combined with the components below

Add
Subtract
Merge
Low
Group

Grouping

Grouped components are also indicated by their own icon and the presence of a plus or minus control to the left of the visibility checkbox. These controls allow you expand or collapse the group to show or hide the group contents, respectively.

Every component exists on a single Level. These levels can be used to organize your modelling process. During the compositing process the contents of a level are combined first before the levels themselves are combined together.

Selection

Components can be selected in 3 ways:

  • By left-clicking on the component's name in the Component Tree
  • By left-clicking on the associated grayscale component preview image in the 2D view
  • By double left-clicking directly on the component in the 3D view

In all cases, the new selection will subsequently be reflected in all three locations. So, for example, selecting a component in the Component Tree will simultaneously cause the associated 2D component preview to become selected in the 2D View, and the same component to become highlighted in red (or green if the selected component is obscured by another component) in the 3D View.

There are, however, some minor differences between the three methods of selection. Also, depending on the circumstances, there may be some advantages to selecting your components using one method rather than another.

Selection in the Component Tree

The component tree works in a similar way to the Window's file explorer. To select a component, simply click on it. To select multiple components, hold down a Ctrl key while clicking on each component you wish to add to the selection. While in this mode, clicking on a component that is already selected will cause it to be removed from the selection.

Pressing a Shift key allows you to select a range of components. Click on the first component in the range to select it, then holding a Shift key and pressing the last component you want selected will select all the components between the first and last selection.

Double-clicking a component or level in the Component Tree will automatically open the Component Properties tool - see the Component Properties section for more information on how to use this tool to modify the selected components.

Right-clicking an unselected component in the Component Tree will select it, and open its pop-up menu of related commands. Any commands you select will apply to this selected component only.

Right-clicking a component that is already selected, and is also one of several selected components, will open a similar pop-up menu of commands. Any commands you select from this menu will apply to all of the currently selected components.

Selection in the 2D View

The 2D component previews behave exactly the same way as vectors or bitmaps. They can be selected by a single, left-click. Several component previews can also be 'shift selected' (see above). Clicking on selected component previews again activates their interactive transform handles. These can be used to move, rotate or stretch the 2D component preview and its associated 3D component.

Selection in the 3D View

Because the left mouse button is used for twiddling the 3D view itself, a single left-click cannot be used for component selection directly. However, Cut2D Pro's 3D view supports most of the standard selection concepts described above, using double-clicks instead. Therefore, to select a component in the 3D view it must be double-clicked with the left mouse button. To select multiple components in the 3D view, hold down a Shift key and double-click each of the components you wish to add to the selection. To access the pop-up menu of commands associated with a component, double right-click it in the 3D View.

Because components may overlap or merge through one another when forming the composite model, you may find that some components become difficult (or are even impossible) to select directly from the 3D view using the double click method. In this case you may use the right click menu. If you right click on a point above the component you wish to select then you are presented with a list of all the components that lie under this point.

Right clicking on a point gives a list of all components under this point. Choosing a component selects this component.

You can also double right-click the selected component (highlighted in red) in the 3D view. The options offered include showing/hiding components, or setting their combine mode within the composite model.

In the 3D view selected object will often be tinted red. On some occasions parts of some components will be obscured by other components. In this case then the red tint will not be seen. The parts of the objects that are obscured will be tinted green so they are still visible from within the 3D view.

The parts of the selected component which are obscured are tinted a different color.

Editing in the 3D View

Many of the dynamic component editing tools can now be accessed directly from the 3D View. Editing the components in the 3D View makes it quick and easy to see the immediate effect of the changes to the Composite Model. To access these editing options a component or components must first be selected. Once selected then either clicking the component again in the 3D view or clicking the Transform Mode icon (Move, Scale, Rotate Selection) will activate the 3D Transform Handles. These take the form of solid and hollow blue squares around the component/s in the 3D View.

Clicking a selected component in the 3D View will activate the Transform Handles.

The majority of these will function in the same way that they do with objects in the 2D View. The additional larger solid blue square below the middle of the bottom edge of the model can be left-clicked to open a floating form that allows access to some of the components properties. This form can be moved if it is covering an important area of the job. From this form you can adjust the Combine Mode, Shape Height, Base Height, Fade and Tilt for the selected component/s. If you edit Fade or Tilt using this form, then when you click the Set button you must click the positions for this in the 3D View.

Clicking a blue square below the component opens a floating Component Property form.

Position in the Component Tree

The position of the component in the Component Tree may affect the resulting combined model. This position can be altered by selecting one or more component(s) and clicking one of the buttons with a blue arrow at the top of the Component Tree. Alternatively, component(s) can be selected and dragged in component tree via mouse. If Ctrl is held when component is being dragged, then the component itself will not be moved, but it will be copied instead and placed at the desired location.

Modeling | Create Component from Bitmap

This tool lets you automatically create a 3D Component from a Bitmap.

If no Bitmap is selected in the 2D View, then a File dialog will open allowing you to select an image file from one of the drives on your computer. This method of component creation bypasses the need to convert the image when importing which potentially reduces the number of color shades, so this second method is the best way to directly convert Bitmap files to components in Aspire.

The Component from a Bitmap is automatically scaled and set to Add to other Components by the software so will typically need to be edited using the Component Properties icon to adjust height or Combine Mode and the Transform tools to adjust its size and position.

Converting selected bitmap

If you have a selected Bitmap in the 2D View this will automatically create a new component derived from that Bitmap, the Component will have the same name as the original image.

Converting without bitmap selected

If no Bitmap is selected in the 2D View, then a File dialog will open allowing you to select an image file from one of the drives on your computer. This method of component creation bypasses the need to convert the image when importing which potentially reduces the number of color shades, so this second method is the best way to directly convert Bitmap files to components in Aspire. This is especially important for 16-bit images.

Modeling | Create Component from Visible Model

The Create Component from Visible Model feature allows you to quickly create a single component which is a copy of the model shown in the 3D View (the Composite Model). The new model created is placed on the active level.

It is common when working with lots of components to find that a number of levels have been used. If, as a final step, you want to edit the models using a tool like the sculpting (which requires the components to be baked together) then they all must be on the same level, however placing the models on the same level may change the appearance of the composite model. In this case we can use the Create Component from Visible Model tool. This resulting component may then be sculpted without any of the previous modelling information being lost.

Consider the following example of a lioness we are modelling, and all of its current levels.

Model Tree
Model

If we want to sculpt this model we must first bake it, but we currently can't bake it because the components lie on different levels. Also, baking them together will mean we lose all our structure that we have carefully built up losing the potential to edit the individual parts. So instead we use the Create Component from Visible Model tool. This creates a copy of what is visible. We can then bake this new component, and we can now sculpt without losing our structure

Model Tree after creating copy
Sculpted Model

Modeling | Create Shape

The Create Shape tool allows the user to create Components based on one or more closed vectors. The vectors can be selected either before the icon is clicked or after the form is open. The user works through the form specifying the profile and strength of the shape and modifying options to govern its height. There is also an option to Tilt the shape on an angle. Once any of the parameters have been defined it can be previewed by hitting .

This shape can be easily changed by altering the parameters in the form and hitting the button to update the preview. Once you are happy with the shape created then you have two choices, to (which will save your current component and start a new one) or the form.

Changing values with the slider on the form will immediately update the 3D view when you release the slider. If you make changes to the edit fields such as Angle or Base height, pressing the 'Space' bar on your keyboard after you have finished entering your value will apply the changes and update the 3D preview or you can hit the button again.

If you select another vector, then the current shape will be discarded, so remember to hit if you want to keep a copy of it.

Shape Profile

There are three different shape types:

Curved

[object Object]
Applies a round profile (dome) to the selected vector/s outline

Angle

[object Object]
Applies an angular profile (pyramid) to the selected vector/s outline E

This will define the angle of the edge of the rounded or angled profile shape - the higher the angle, the steeper the shape. Angular shapes can have a maximum angle of 89°. The slider bar to the right can also be used to change this as well as typing a specific angle into the form.

Flat

[object Object]
Applies a flat profile to the selected vector/s outline

Base Height

Specifies the height of a flat 'base plane' added below the profile you have chosen.

Final Height

No Limit

Checking ✓ this option lets the combination of the size and shape of the vector and the specified profile values govern the final height of the shape.

Limit to Height

Checking ✓ this option limits the height of the shape by flattening it off at the value entered in the Height area of the form which becomes active once this option is selected.

Scale to Exact Height

Checking ✓ this option limits the height of the shape by scaling the shape up or down while retaining its general specified profile. It is scaled to the height entered in the Height area of the form which becomes available once this option is selected. The slider can also be used to change the final height.

The Base Height value is not included or controlled by the Final Height setting and if specified will be added to this value to give the total height of the component being created.

Tilt

When this option is checked ✓ the user can set a direction and angle to tilt the shape up at an angle in Z. The first part of this operation (once the option is checked ✓) is to press the button - then click two points in the 2D view.

The first click specifies the point which will remain at zero (the pivot point of the tilt).

The second click specifies the point that will be tilted upwards by the specified angle (the point that will be raised up).

The default angle (10°) can be edited by clicking the arrow next to the value and using the slider or by typing in a specific value and hitting the Space Bar on the keyboard to apply the angle.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Modeling | Create Texture Area

The Create Texture Area tool assists in the creation of components with a repeating pattern or texture. It requires a single component and optionally one or more closed boundary vectors which define the region in which the tiling should take place.

The Create Texture Area form is accessed from the modelling tab.

The first step is to select the component you wish to be tiled. If you want to restrict the tiling to a region then you should also select one or more closed vectors which will represent the boundary when the texture is created. If no boundary vector is selected then the tiling will fill the entire job space.

The Create Texture Area form contains options to adjust the spacing, overlap, positioning and symmetry of the texture which are discussed below. When you click the Apply button then the software will create a Component based on the settings in the form and any vector you may have selected for the boundary.

At this moment the original selected Component will be made invisible to avoid confusion with what you can see in the 3D View.

Once you click then this will effective fix the basic outline or silhouette of your Texture Area either based on the selected vector or the job area. It is possible to edit the size, position and rotation of this but if you wanted to change to a different border shape then you would need to start again with a new selection.

Seed Component
Seed Component
Tiled Result
Tiled Result

By default the form has Transform Object selected at the top. In this mode you can click on the Texture Area Component and use the drag-handles to move, scale or rotate it. Note that this will not change the size of your Tile (original seed Component). To change the size of the Tile you would use the Edit Textured Area Component option which is covered further down in this document.

Note

Create Texture Area effectively fits a box around the original object in order to apply the settings from the form, it can be useful to keep this in mind while editing the values. It's simpler to only edit one value at a time to keep track of what is happening as the Texture Area is built.

Spacing

The spacing edit box or sliders can be used to control the degree of spacing between the tiles in a pattern component. You can adjust the spacing between the components horizontally and/or vertically. The amount of horizontal spacing is given in terms of a percentage of the width of the tile component. The amount of vertical spacing is given in terms of a percentage of the height of it. To control the amount of spacing, use the two sliders in the box marked Spacing. Drag and release the slider to set the percentage, or alternatively type an exact amount into the edit box above and either hit or press the Space bar on the keyboard to update the result. You can enter both positive and negative values. Positive spacing values open gaps between the objects in the texture and negative spacing has the opposite effect making the tiles overlap one another as shown below.

Shape with 25% X and 25% Y spacing
Shape with -25% X and -25% Y spacing
Shape with -25% X and -25% Y spacing

Translation : X/Y Shift

The X/Y shift option can be used to move all the tiles in alternate rows horizontally or alternate columns vertically by the specified amount. As with the spacing, the X/Y shift is given as a percentage of the size of the component in the appropriate dimension and can be adjusted using either the sliders or the edit boxes. For example entering a shift value of 50% horizontally (X) would move the second row over by half the width of the object, the third row would be as the first, then the fourth shifted, this shift would also be applied to every other row after that within the Textured Area. Similarly entering a value of 50% for the vertical shift (Y) will move every other column up by half the height of the object.

Shape with 50% X shift
Shape with 50% X shift
Shape with 50% Y shift
Shape with 50% Y shift

Reflection

The reflection tool consists of four buttons. Each button represents one tile in a mini-group of four, starting from the lower left copy which is represented by the original Tile. Each button has 4 states of reflection, each time the button is clicked, the icon representing the button will change to show the current state. Click to update the Texture Area Component with your new choice.

No reflection
No reflection
Horizontal reflection
Horizontal reflection
Vertical reflection
Vertical reflection
Both horizontal and vertical reflection
Both horizontal and vertical reflection

Editing an Existing Texture Area

When you have created a pattern you can edit the size of the individual Tile component you are creating a pattern from by selecting the Edit Textured Area Component option at the top of the form. Within the 2D View this will then put an orange transform box around the lower left component in the pattern. You can alter the size of this by left clicking on one of the handles and dragging it to size, when you let go this will update the pattern to fit the new size within the Texture Area boundary. You can also move the location of this Tile by clicking the center node and dragging it with the mouse to a new location. This again will change the layout of the pattern.

Note

It is not currently possible to scale or move the Tile using drag handles in the 3D View.

Pattern in Edit Texture Area Component Transform Box Appears
Pattern in Edit Texture Area Component Transform Box Appears
Pull handle on Transform Box to Alter Size and the Pattern Updates to the New Size
Pull handle on Transform Box to Alter Size and the Pattern Updates to the New Size

A Texture Area component will remember that it is in a special state and not a standard component. This means that they can be further edited using the Texture Area form even after Closing and re-entering the function. To edit an existing Texture Area component, select it and then open the Create Texture Area tool. Alternatively, open the Create Texture Area tool and then select the existing component. This will then let you continue to make changes to it using the form.

Resizing

Texture Area components do not behave like standard components when they are scaled in X or Y. When a Texture Area component is resized, then this resizes the boundary in which the tiling takes place so the size of the individual Tiles will not change, just the area that they are covering will be updated.

Typical baked component resize - shapes scale
Typical baked component resize - shapes scale
Texture component resize - shapes do not scale
Texture component resize - shapes do not scale

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Modeling | Create Vector Boundary From Selected Components

This icon can be used to create a vector around the outermost boundary (silhouette) of one or more selected components. The most important use is to generate a vector that can be selected as a toolpath boundary, particularly for 3D Roughing, 3D Finishing and also Profile (cutout) toolpaths.

Cut2D Pro will create one or more closed vector boundaries around the edge of the selected components. If more than one closed vector is required to create the boundary, these will be created as a group to make it easier to select them. They would need to be ungrouped before they could be edited individually.

Mirror Mode

You can use this tool to create a vector boundary for a composition you have created in Mirror Mode. Simply select the components that are visible in the 2D View and apply the vector boundary.

Modeling | Create Zero Plane

Creates a component that is the size of your job setup with a height of Zero.

Modeling | Emboss Component

Embossing a component can be used in some cases to reduce the height of a model while preserving important surface detail as an alternative to the standard method for scaling a components height using the Shape Height option on the Component Properties form. A component must be selected before the tool can be used.

The images below show the same model, both results are scaled to ten percent of their original heights. The image below left was created using the standard Shape Height scaling from the Component Properties form and the image below right using the Emboss function.

Original model
Original model
Embossed Model
Embossed Model

Scale Height

Use the Scale Height slider to adjust the final height of the component.

Detail Smoothness

Since the results of the initial detail scaling can be noisy the Detail Smoothness slider can be interactively adjusted to improve the visual quality of the result. In general, the greater the Scale Height the more Detail Smoothing needs to be applied.

Remarks

The Emboss tool is a very powerful feature but will not provide ideal results on every type of 3D model. Although it's possible to use the Emboss tool on models created in Cut2D Pro and other low-relief imported designs (such as the clipart), it's important to understand its intended use is with data from imported, full 3D (high relief) models and typically the best results will be obtained with this type of data.

Modeling | Export Model as an STL File

The STL file format is an industry standard for representing 3D models as meshes made up of a skin of triangles. It is a very robust way of exporting a version of your 3D composite model to external applications or even Rapid Prototype (RP) machines. Models can also be exported as an OBJ file, which includes the component colors and is primarily used for ray-traced rendering of your model.

Limit Triangles By...

In general, triangle meshes are not able to hold as much detail as Aspire's 3D Components. As a result, you must choose which strategy Aspire will use to reduce the detail in your STL file.

Note

When exporting the rotary model, currently there is no control over the number of triangles and the mesh will be exported at the highest quality. That means that the generated file will have a considerable size.

Approximate tolerance

Using this option the quality of the mesh is defined by how closely you allow the software to approximate the model. The smaller the number the better the detail and smoothness of the model but the larger the memory size of the file will be.

Maximum number of triangles

Using this option the quality of the mesh is limited by how many triangles you specify here, the larger the number the better the detail and smoothness but the larger the memory size of the file will be.

Back face of triangulation

The Composite model does not have a defined back face, because it is generally unnecessary for conventional 3-axis CNC machining. When converting your composite model to a 3D mesh, however, it can be useful to form a closed mesh by creating a back face automatically.

Leave Open (No Back Face)

This creates a mesh with an open back. This creates a shell with the 3D shape on its face and an open back side.

Note

When exporting the rotary model this option will result in a mesh without caps at the ends.

Close with inverted front

This creates a mesh with a copy of the front of the model on the back. This is used when a solid 2 sided model is needed for output. An example of this might be a 2 sided fish.

Note

When exporting the rotary model this option is not available.

Close with a flat plane

This creates a mesh that has its back sealed off with a flat plane. This type of closed model may be required by Rapid Prototyping (3D Printing Software) to allow the part to be prepared for the production process.

Note

When exporting the rotary model this option is not available.

Close with other side (two-sided jobs only)

In the case of two-sided jobs, this option can be selected. It will triangulate both sides of a job and produce a single closed mesh.

Note

When exporting the rotary model this option is not available.

Close sides

This option is only available for rotary jobs. When it is selected the created mesh will have caps on the ends.

Triangulate

When the options for the mesh have been selected then clicking will actually calculate the mesh and display the result in the 3D View. If this does not look correct (such as not being detailed enough) then the options can be changed and this button clicked again to re-calculate the mesh.

Num Tri Created

Once a mesh has been created, this field reports how many triangles it comprises. The more triangles are used, the larger the file size and the more difficulty external applications may have in manipulating them.

Maximum Error

This field indicates the worst deviation of a mesh triangle from the original 3D model.

Draw shaded triangulation

The triangle mesh can be viewed in wireframe or shaded modes using this option.

Save Triangulation...

Once the mesh looks correct, then clicking this button enables it to be saved onto your computer as an STL format file by default. The file save dialog also allows the selection of Wavefront (*.obj) and POV-Ray Scene (*.POV) as an alternative triangle mesh format using the Save as type option.

Note

When saving an obj file, an additional material (*.mtl) file and texture image file (*.jpg) will also be created - all three files will be required when opening the obj file in a 3rd party modelling or rendering package.

Modeling | Extrude and Weave

The Extrude and Weave feature is a very powerful and flexible modeling tool. It uses one or more vector drive-rails to define the path that the shape will follow, this allows you to extrude either vector cross-sections or 3D Components along these vectors to create the model.

The first stage is to select the drive rails and then choose whether you want to use either vectors or Components to extrude along your curves. There are many options both on the form and under the context sensitive right-click menus that can be used to control the shape that is created.

Drive Rail Selection

From the 2D View use the mouse to select one or more open or closed vectors you wish to use as the drive rails for you to extrude or weave along. Then click the button.

In the 2D view your rail vectors will be highlighted orange and now show a green square (start node) indicating the start of the vector from which the extruded shape will begin, and arrow markers along its length to show the direction of the extrusion.

The default start point and direction shown may not be what you intended. To change the direction, right-click with the cursor on the vector line and select Reverse Rail from the context sensitive menu, you will now see the arrows on the drive rail change direction. On a closed vector you can change the start point by placing the cursor over an existing node in the drive-rail vector, right-clicking and selecting Make Start Point or you can right-click anywhere on the vector and select Insert Start Point to create a new node which will become the start point.

Note

Remember that you can hold down a Shift key while left-clicking on vectors in the 2D view to include more than one vector in the selection.

The button can be used at any time to empty your current selection. This will delete your current shape and deselect all the drive rail and cross section vectors. This can be used if you do not want to create a Component before you exit the form or if you want to select new vectors in the 2D view to use as the drive rail for your shape.

Using Vector Cross Sections

In this section of the form you can select whether to use vector cross sections or Components to extrude along your drive rails, select either Use Vector Cross Sections or Use a Component to make your choice.

Cross Section Selection

The next step is to select one or more cross-section vectors to sweep along your rails to form a 3D shape. In order for vectors to be used as valid cross-section shapes, they must be open.

Select a vector that you wish to use as a cross-section in the 2D View by left clicking on it with the mouse.

If you are using just a single cross section then you just need to make sure it is selected and then can proceed with the other settings in the form and calculate your shape. If you want to edit cross section positions or add more than one cross section then you will need to attach them to the drive rail.

Select a vector that you wish to use as a cross-section in the 2D View by left clicking on it with the mouse. Now click on the drive rail to attach the cross-section to that vector.

As you move the mouse over a selected drive rail it will indicate with a check mark ✓ that it is a valid place to add the cross section. Once a cross-section has been successfully attached to your drive rail, the 2D view will show a preview using line markers to indicate how the cross section will be positioned when it is extruded.

Two Cross-Sections are always created when you attach the first cross-section to the drive rail - one at the start and one at the end. The intermediate lines along the entire length of the rail indicate how the shape will flow between the defined cross sections. You can click the button to create your 3D swept shape.

Using multiple cross-sections

It is possible to extrude between multiple cross section vectors along a drive rail blending from one vector shape to another.

Adding Cross-Sections

To add a new Cross-Section to an existing extrusion, simply select an open vector in the 2D View that you wish to use as a cross-section. With the vector selected, click on the point along the rail to which you wish it to be attached. A new Cross-Section will be inserted at this point. On applying the change, the resulting 3D sweep will blend seamlessly between all the defined Cross-Sections along the rail.

Note

To help differentiate which cross section is being used at each location the software will indicate a colored node at one end of each cross section and place the same colored node on the preview position. This node also indicates the direction the cross section is being 'hung' across the curve. The same cross section vector can be used in multiple locations along the drive rail.

In some cases it may be advantageous to add a cross section at all node positions on a drive curve, for example on a closed rectangular border. This can either be done manually, or automatically after you have added the first Cross-Section by right-clicking on the cross section you wish to duplicate and selecting Add To All Rail Nodes. This will add that same cross section to every node on that specific drive rail vector.

Removing Cross-Sections

To remove a Cross-Section, position the cursor over the cross section and click the right mouse button. Select the option to Delete Cross Section from the menu.

If you remove the start or end Cross-Section and fail to replace them with a new cross-section vector then the preview will no longer show intermediate lines to that point on its length. This means the shape will start or stop at that cross section and not go all the way to the start/end of the line. You can either add a new cross section or drag an existing one to that position if you need to resolve this.

You can remove all the Cross-Sections on a drive rail by positioning the mouse arrow over a part of the curve that does not contain a cross section. This will bring up a different context sensitive menu and you can select the options to Remove All Cross Sections.

Create sharp corners

If this option is checked, ✓ then the tool will create a sharp corner in the Component where there are discontinuities in the drive rail vector. When unchecked the shape will be rounded as it goes around the discontinuity. Below you can see a rectangular drive curve with a simple cross section being extruded around it, the one on the left has the Create sharp corners option selected and the one on the right without.

Create sharp corners checked ✓
Create sharp corners checked ✓
Create sharp corners un-checked
Create sharp corners un-checked

Sweep between spans

When checked ✓ this option will ensure that as the shape is extruded that it goes from a particular span/node in one cross section to the same span/node on the next cross section. For some applications this can give the user more control over the way the shape flows.

Using the above vector selection, the shape below left will be created with Sweep between spans checked ✓ and the shape on the right is created with the option un-checked. Note that on the left hand picture the crease in the shape goes from node to node in the cross sections as the spans flow exactly from one to the next. On the second picture the shape just linearly flows from one cross section to the next evenly with no additional control.

Sweep between spans checked ✓
Sweep between spans checked ✓
Sweep between spans un-checked

Smooth transition through the Cross Sections

As the extruded shape passes through each cross section the default is for it to flow smoothly through the profile. This can be edited by right-clicking over a cross section and unchecking the Smooth option. The middle node on the cross sections preview in the 2D View will be blue if it is smooth and white if it is un-smooth.

[object Object]
Profiles for Extrude

Using the above vector selection, the shape below left will be created with the Smooth option checked ✓ and the shape on the right is created with the option un-checked. Note that on the left hand picture the shape flows smoothly through each span, on the second it goes directly from cross section to cross section in a straight transition.

Smooth checked ✓ on all cross sections
Smooth checked ✓ on all cross sections
Smooth un-checked on all cross sections
Smooth un-checked on all cross sections

Extrude and Weave Components

The Extrude and Weave feature also allows the option to use a 3D Component instead of using vector cross sections to define the shape being created. To activate this feature choose the Use a Component option under the Cross Sections / Sweep Interior section of the form.

Once this option has been selected then you need to select a single Component that will be used for the operation. This can only be done within the form and not from either of the views or the Component Tree. Use the arrow at the side of the name in the drop down list to access a list of all the Components and select the one you want to use. By default the first Component name in the Component Tree will be shown in this section of the form. If the form is opened with a single Component selected, the selected Component will be the default in the list. Once selected a preview of the extrusion will be shown in the 2D view.

The orientation of the Component in your part will control how it flows along the vector. The direction along the X-axis of your Component will govern how it flows positively along the drive curve. Another way to think of it is you need to position your Component so it faces from left to right to orient how it will point along the curve.

Once your Component has been selected from the list you need to choose whether it will be used as a single copy stretched along the curve or repeated multiple times at its original size.

Stretch to drive rail length

Picking this option will take a single copy of the Component and stretch it along the full length of the selected drive rail vector.

Fill with multiple copies

Selecting this option will keep the Component at its original size and repeat it along the drive curve. Specifying an Overlap value will set each copy of the Component to overlap the previous one by this percentage of its length. Each overlapping piece will be merged together. In addition to overlapping the parts you can also check ✓ a box to flip alternate copies of the Component. This will flip every other copy of the original as if it had been mirrored vertically.

Fill with multiple copies 0% Overlap
Fill with multiple copies 25% Overlap
Fill with multiple copies 25% Overlap
Flip alternate copies 25% Overlap
Flip alternate copies 25% Overlap

Weave under/over at crossings

With either vector or Component based extrusions you have the option to activate the Weave part of the function. This gives the ability to raise and lower the extruded shape at positions where the drive rail vector or vectors cross over. The effect of this is a Component that appears to be weaving the extruded shapes as you can see below.

Preview of weave vector selection
Preview of weave vector selection
Result of weave with 70% Z Under and 130% Z Over
Result of weave with 70% Z Under and 130% Z Over

The order of the weave is determined by the direction of the first vector picked as part of the drive-rail selection. To change the order of which overlapping positions are raised up and lowered you can right mouse click on the first drive rail vector you selected and choose the option.

There are two options to control the way the shape is scaled at each overlapping point in the drive rail vectors, Scale Shape and Add Base.

Scale Shape

The Scale Shape option uses the percentage values entered into the form to scale the height of the original shape up and down at the cross-over positions. For example entering a Z Under percentage of 50% will force the locations which are being weaved under to be half their original height. Entering a Z Over percentage of 150% would force the locations of the shape which are being raised as they weave to be 1 ½ times their original height. This will distort the cross sections or Components to stretch or squash them.

Scale Shape - 80% Z Under and 120% Z Over
Scale Shape - 80% Z Under and 120% Z Over
Scale Shape - 30% Z Under and 150% Z Over
Scale Shape - 30% Z Under and 150% Z Over

The Scale Shape option will give a natural looking weave but for certain shapes will mean the detail in the shape may become heavily accentuated or reduced at the overlaps. In these situations the Add Base option may create a better result.

Add Base

The Add Base option will retain the height of the original cross section or Component and raise it up adding material under the shape depending on the percentage values indicated. This will typically create a higher final Component than using the Scale Shape option but gives a consistent shape to the strands of the weave.

Scale Shape - 0% Z Under and 50% Z Over
Scale Shape - 0% Z Under and 50% Z Over
Scale Shape - 0% Z Under and 100% Z Over
Scale Shape - 0% Z Under and 100% Z Over

Scale to Exact Height

Checking ✓ this option scales the shape calculated so its maximum height is the value entered in the Height area of the form.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Editing vectors while using the Extrude and Weave tool

It is possible to make edits to the vectors that you have selected while using the Extrude and Weave tool. To do this you can click in the whitespace of the 2D View to ensure you have focus on that window. Then on the keyboard hit either N to go into Node Editing mode or T to go into Transform mode.

You will notice the drive rails and cross sections will become deselected and the button will change to say . You can now make edits to the vectors using the dynamic Node Editing and Transform functions in the 2D view. When you are happy with your changes you can click on the button and the vectors will be selected in the same order they were before. Now you can click the button to create a new shape based on the edited vectors.

Modeling | Import 3D Model into Single or Two Sided Job

Initial Orientation

Choose one of the 6 options to determine the most suitable direction on the model that defines the top surface (upper Z) that you want to use when it's converted into a Component.

You can also use the five options for Rotation about Z Axis to modify the position of the part being imported at this stage.

Interactive Rotation

The default choice XYZ-View allows you to left-click in the 3D View with the mouse to rotate your view so you can examine the part from different angles. Using this will not change the orientation of the part for import. If you select one of the other four options above the word Model then this will adjust the actual positional orientation of the imported part. Choosing the XYZ option will allow rotation around all three axes simultaneously, X, Y or Z will only allow rotation around the specified axis. This is also done using the left-click in the 3D View with the mouse.

Model Size

Lock XYZ ratio

Un-checking this option allows the model to be distorted from its original shape. This means independent X, Y and Z sizes can be entered. Leaving it checked ✓ fixes the ratio so it cannot be distorted. Instead it will automatically scale the other axes as you enter new values for X, Y or Z.

Apply

Applies the values you have entered for the X, Y or Z dimensions.

Many mesh files do not inherently have the units that they were made in embedde in the files, so the software is not able to tell if the files are supposed to be inches or metric, they will just have a particular value. Therefore it is quite common to need to scale the part from inch to metric or vice versa. If you import your model and you wish to work in inches and the file seems very large or if you work in Metric and the file seems very small then you will probably need to use the Scale mm/inches option. The next two items on the form cover this need.

Units

Choose the unit of measurement (mm or inches) that you are working in, within the part the file is being imported into.

Changing the units will result in resizing the model. For example, if you had 5x5 mm dimensions, they would become 5x5 inches so the model becomes a lot larger.

Scale mm/inches

Scales the X, Y and Z values up or down depending which Unit option is selected. If mm is selected then the software assumes you want to scale the values up so multiplies the current values by 25.4, if inches is selected it assumes you want to scale the values down and divided them by 25.4.

Zero Plane Position In Model

This slider bar determines where the 3D model will be cut-off when converting to a Component. You can move this up and down with the mouse or use the Middle or Bottom buttons to locate the plane in the correct position.

Note

Anything in the original model which is an undercut (goes underneath another part of the 3D model) will be discarded and a vertical wall will be created down to the plane from the silhouette (looking down Z axis) edge of the model.

Discard data below zero plane

Checking ✓ this will remove any data below the original Zero level within the imported 3D model. If the model is effectively a negative model such as a dished or recessed design with a flat plane then you should uncheck this option to make sure you retain the 3D data below the plane.

Create both sides

If you are working in a 2 sided setup you can check ✓ this option and two components will be created - one looking down the Z axis from above to the zero plane and one looking up from below. Each side of the model will go onto a side. This will provide you with the geometry that can be edited to cut the original imported 3D part as a 2-sided job.

If you were importing a model that contains a non-convex surface for instance a bowl you can import the entire model on each side by sliding the slicing plane all the way to the bottom.

Center Model

The button which will move the center of the model's bounding box to datum position (XYZ zero). This is particularly useful if you intend to unwrap a model for rotary machining. This may change the Zero Plane position in the model.

Apply Perspective along Z

Checking ✓ this will enable you to apply a perspective distortion to the model along the Z axis by using the slider. Points on the model closest to the observer will become further apart as the distortion strength is increased - this makes the model appear as if it is coming out of the screen.

OK

Creates a 3D Component based on the settings in the form, the Component will have the same name as the imported file. If you selected 'Create both sides' you will have two components with the name of the imported file followed by the suffixes -Top and Bottom.

Cancel

Cancels the Import function and returns to the standard Modeling Tab icons.

Modeling | Import a Component or 3D Model

This command opens the File Open dialog window, allowing existing Cut2D Pro files (CRV3D extension) and importable 3rd party 3D files to be selected and opened. If you select a 3rd party 3D model format, the Orientate Model form will open (see below) to allow you to manipulate the 3D model before it is converted into a Component.

CRV3D

3D data from files previously created and saved in Cut2D Pro will be opened and a new single Component Created (from all the visible 3D Components in the file when it was saved). The new Component will have the same name as the file. This will be imported at the size and position the part was saved in the original file.

3DCLIP

3D Clipart files are exported from Cut2D Pro. This format maintains the component structure of clipart pieces at the time of saving, so will import all the components comprising the clipart piece. This will be imported at the size and position the part was saved in the original file.

V3M

V3M is a proprietary file format developed by Vectric for Vector Art 3D and Design and Make. Files in this format can be purchased from www.vectorart3d.com and www.designandmake.com and when imported into Cut2D Pro will create a new Component with the same name as the file. This will be imported at the size and position the part was saved in the original file.

STL

This is a standard format for complex 3D models, based on a triangular mesh. STL files can be exported from many 3D design software programs such as Rhino. These models can be completely 3 dimensional (i.e. have a front, back, etc.), this means that when this type of file is opened that it must first be sized and oriented before a Component can be created (Cut2D Pro only represents base-relief so cannot work with a completely 3D object). Once the file becomes a Component it will have the same name as the original STL file. This file type will need to be imported using the Orientate 3D ModelCut2D Pro.

DXF

3D DXF files from AutoCAD and many other CAD orientated modeling packages, these must be 3D meshes and not just wireframe data of the models vertices. This file type will need to be imported using the Orientate 3D ModelCut2D Pro.

3DS

A native format from 3D Studio Max and many other animation orientated modeling packages. This file type will need to be imported using the Orientate 3D ModelCut2D Pro.

OBJ

A native format from Wavefront and many other animation orientated modeling packages. This file type will need to be imported using the Orientate 3D ModelCut2D Pro.

SKP

A native format from the SketchUp modeling package. This file type will need to be imported using the Orientate 3D ModelCut2D Pro.

Note

If you wish to read data from a 3D digitizer or scanning device then STL is typically the best format that should be used to import the data. Many software packages that work with a scanner offer an STL export option, if not then a third party software program may be required to convert the data to an STL model.

Modeling | Importing a 3D Model into Rotary job

Imported model type

Allows the nature of the imported model to be specified. Depending on the selection, the form will change to allow the most appropriate workflow. You can choose from the following model types:

  • Full 3D model - a model that is suitable for rotary machining as is,
  • Flat model - a model that is only suitable as a part of design, similar to clipart provided with Cut2D Pro.

Initial Orientation

The purpose of this section is to roughly position the imported model within the material block. One can choose one of the 6 options to determine the most suitable direction on the model that defines the top surface (upper Z). This can be combined with one of the five options for Rotation about Z Axis.

Note

The software will try to guess the initial orientation that seems to be appropriate for the model, based on the model type selected in step one.

Interactive Rotation

This section can be used to fine-tune the model position in relation to the material block. The default choice XYZ-View allows the usual use of the mouse to rotate the 3D View, so the imported part can be seen from different angles. While this mode is selected, the orientation of the part will not change. Selecting one of the other four options above the word Model will enable adjustment of the actual positional orientation of the imported part. Choosing the XYZ option will allow rotation around all three axes simultaneously. Selecting X, Y or Z will only allow rotation around the specified axis. It will also automatically switch the 3D View to show the part from that axis.

Note

Selecting a different initial orientation will cancel any adjustments made by using Interactive Rotation.

Rotation Axis Movement (Full 3D model only)

This section can be used to adjust the position of the model in relation to the rotation centerline. By default Cut2D Pro will position the model in the center of the material block, so the material is used more efficiently.

When the Off option is selected, panning the 3D View will happen in the usual manner.

When the On option becomes selected, using the 3D View panning controls will move the rotation axis instead.

Model Scaling (Full 3D model)

This section allows the model scale to be adjusted as desired. The model bounding cylinder (blue) will be displayed around the imported model in the 3D View. The scaling is performed by means of length and diameter of the bounding cylinder. When the model orientation within the material block changes, so does the bounding cylinder. If that happens, the reported size of the model will change, although the model may not have been scaled.

Model units

By default Cut2D Pro assumes that the imported model is using the same units as specified during job setup. If that is not the case, the model units can be changed.

Note

If the model units are different than those selected during job setup, the imported model will be converted to use the units selected during job setup.

Lock ratio

When this option is selected, all scaling operations will maintain the current ratio between model length and diameter.

Scale model to fit material

This option can be used to resize the imported model so it will fit in the material block as defined during job setup.

Reset to Original Size

This option undoes any scaling applied to the model (apart from unit conversion), regardless of the model orientation.

Resize material block

When this option is selected, the project's material block will be resized to match the final dimensions of the imported model.

Model Scaling (Flat model)

This section allows the model scale to be adjusted as desired. A flat material block is displayed and the scaling can be performed by means of length in each of the three axes (X, Y and Z).

Model units

By default Cut2D Pro assumes that the imported model is using the same units as specified during job setup. If that is not the case, the model units can be changed.

Note

If the model units are different than those selected during job setup, the imported model will be converted to use the units selected during job setup.

Lock ratio

When this option is selected, all scaling operations will maintain the current ratio between the model length in each of the three axes.

Scale model to fit material

This option can be used to resize the imported model so it will fit in the material block as defined during job setup.

Reset to Original Size

This option undoes any scaling applied to the model (apart from unit conversion), regardless of the model orientation.

OK

Creates a 3D Component based on the settings in the form, the Component will have the same name as the imported file.

Cancel

Cancels the Import function and returns to the standard Modeling Tab icons.

Modeling | Offset Model

The Offset model tool creates a 3D offset of the composite model.

To use the tool, specify the distance that you want to offset the model.

Click on the button to see the results of the offsetting.

Click to proceed or click to exit the form.

The Clip Z values to the Zero Plane option will ensure that the final result will always be positive. When used on models with areas that end up lower than the zero plane these parts of the model will be removed leaving only the positive values. This can be helpful when you have a flat plane as part of the model to avoid it being effectively lowered by the offset amount.

Using this function you can offset with either positive or negative values.

Original model
Original model
Negative Offset
Negative Offset
Positive Offset
Positive Offset

Note

Clicking the Preview button repeatedly will apply your chosen offset multiple times. Click the Cancel button to remove all effects of the previews.

Modeling | Replace Below

This feature allows you to trim (or flatten) the bottom off a component or multiple components. This could be useful if you've imported an STL model that has some undesired thickness, for example, when it has come from a 3D scan. Also, sometimes you could end up with an undesired negative part of the components (when sculpting, or combining with a deep subtracted model). This tool will allow you to remove anything below a certain height, and (optionally) drop the model by that height.

The result of the operation will be a component that will appear in the Component Tree.

  • If only a single component is selected, it will be replaced.
  • If multiple components are selected (or a level with more than one component is chosen), they will be baked into a single component, then the operation will applied to the baked component.
Original model
Model after applying Replace Below tool

Note

Select one or more components, or use the active level to get started.

Modeling | Scale Model Height

This tool applies a global scaling to your final composite model. This allows you to accurately fit a design within the available material or to manage the depth of cuts required, without having to individually adjust the depth of each of the contributing Components.

Scale Both Sides

This option can only be selected when working within a 2 Sided Setup. Checking ✓ this option enables you to scale both sides of the model. If this is unchecked then you are only scaling the model of the side you are currently working on.

Scale Height

This slider will allow the user to increase and decrease the height of the model as a percentage based on its original height (when the Scale tool was selected).

Set Exact Height...

Clicking button lets the user define a specific value (in the current working units) for the height of the model, rather than use the proportional slider. If you are working in a two sided environment you have the option scale both sides. Checking ✓ this option enables you to scale both sides of the model. If this is unchecked then you are only scaling the model of the side you are currently working on.

Apply/OK

Exits the dialog keeping the changes made to the Model.

Close/Cancel

Exits the dialog discarding the changes made to the Model.

Modeling | Sculpting

The Sculpting function in Cut2D Pro is a very powerful way to edit (or create) 3D shapes. It allows the user to perform truly dynamic interactive editing of 3D Components. Once activated, the user chooses from a variety of tool options which determine how the model will be changed and then uses the mouse (or a pen tablet) to actually edit the 3D model. This is done in the 3D view and requires the user to click and move the mouse cursor in the area of the model they want to apply the tool. The best way to understand this tool is to actually try it and to watch the Tutorial Videos that are supplied with the software as it is very much a visual tool (which is what gives it its power).

One or more Components can be selected for Sculpting. If you select multiple shapes or a Component Group then the software will need to Bake your selection into a single Component, if applicable you should ensure you have a safe copy of your selection before proceeding.

In addition to components, you can also select bitmap. The bitmap will be overlaid on the sculpted model. This is useful when sculpting based on the photo.

Tool

One sculpting tool at a time can be selected by clicking the option from the form or using the shortcut keys (numbers 1-6 displayed next to each option):

Smooth

As the user moves the mouse back and forward over the 3D model the area under the red cursor will be smoothed out to average the high and low areas of the model.

Smudge

As the user moves the mouse from one place to another on the 3D model the material under the red cursor will be dragged, similar to smudging a piece of clay with your thumb. In Cut2D Pro it means that going from a high to low will pull the higher material into the lower and vice-versa.

Deposit

As the user moves the mouse over the 3D model the area under the red cursor will have material added to it to increase its height.

Remove

As the user moves the mouse over the 3D model the area under the red cursor will have material removed from it to decrease its height.

Undo Brush

As the user moves the mouse over any area of the 3D model that has already been sculpted then the area under the red cursor will be gradually returned to its original state. This can be used to undo some of the sculpting if you make a mistake.

Note

If you press the 'shift' key with the Undo Brush selected you can erase the section of the model under the cursor completely, this is a useful way to tidy up the edge of a shape or delete specific parts of a component.

Alternately you can use the Key combination Ctrl+Z to undo the last move that you made without using the Undo Brush.

Twiddle

Normally when in the 3D View you can twiddle (rotate) the direction of the view by left clicking and moving the mouse. In the Sculpting mode the left click is what activates the sculpting so cannot be used for twiddling the view. Selecting this option allows the user to twiddle the view as normal before returning to one of the other sculpting tools. A Short-Cut to this while in the sculpting is holding the Alt key while holding the left mouse button and moving the mouse.

Diameter

This slider will allow the user to control the size of the sculpting cursor (red circle). This value can also be changed while sculpting by rolling the 'wheel' on a roller mouse, pressing control while rolling the wheel will change the diameter in smaller increments.

Strength

This slider controls the strength of the tool that is currently selected. The higher the strength the more effect the tool will have as the cursor is moved over the model. The strength can also be adjusted by rolling the mouse wheel while pressing the Shift key if you have a roller mouse.

Smoothness

This slider controls how smoothly the selected tool will manipulate the model. A higher smoothness setting will create a more gentle transition while a lower smoothness setting will create a jagged and potentially distorted effect.

Preserve Transparency

This option is checked ✓ by default when you first go into the Sculpting. Leaving it checked ✓ will mask the sculpting so it is only applied within the existing boundary of the component. This stops the edges being blended into the background. It is called Preserve Transparency as the background is represented by a transparent (lighter colored) flat plane around the edge of the 3D component. Un-checking this option allows the user to sculpt the part into the modeling plane if the shape needs to be changed to go outside of its original edge or if the edges need smoothing into the background. Pressing the 0 key while sculpting is a shortcut to toggle this option.

Show Grayscale Background

Exposes the selected component without entirely hiding the other components: they are displayed as a grayscale image on the sculpting screen.

Mode

The sculpting mode defines how the tool is applied to the model in terms of the heights of the shape under the sculpting cursor. The Raise option is good for filling in holes and the Lower option is good for eliminating spikes in a model. A good example of need for this may be if the user was working with 3D digitized data which had been imported from a scanner (e.g. as an STL model).

Normal

Selecting this option means that the sculpting operation will average the high and low points under the cursor dragging them up or down as appropriate.

Raise

Selecting this option will maintain the highest points under the cursor when smoothing or smudging only allowing material to be added (based on the currently selected tool).

Lower

Selecting this option will maintain the lowest points under the cursor when smoothing or smudging only allowing material to be removed (based on the currently selected tool).

Overlay Image

If bitmap is selected when opening this tool, it will be overlaid on the sculpted model.

Overlay image opacity

Controls how translucent the overlaid image is.

Show overlay image

Allow to quickly toggle between overlaid image being visible or not. This allows the user to work with overlaid image hidden and only displayed periodically to guide the sculpting process.

This option can also be accessed by pressing the O key.

Presets

Selecting a preset from the drop down list will restore the sculpting tool settings previously stored within it. This is a quick way of switching between commonly used settings. Selecting <Add new preset...> from the list is an alternative way to create a new preset.

Add

Clicking the button will save the current sculpting tool settings in a preset. You will be prompted to enter a name for the preset. If a preset with the same name for the same tool type already exists then you will be asked if you would like to overwrite it.

Remove

Clicking the button will remove the preset currently displayed in the drop down list.

Changes

Sculpting is a very iterative process and frequently as the user progresses, they will want to either get rid of a recent change, or will want to save the changes they have made and continue sculpting. The options under Changes in the form allow the user to do this.

Keep

Clicking the button will internally save the sculpting changes made so far. This should be clicked if the user is happy with the sculpting so far and wants to keep it but also wants to continue to sculpt the model.

Discard

Clicking the button will discard all the changes made with the sculpting tools back to the stage that the Keep button was last clicked. If the Keep button has not been clicked within a particular sculpting session then all the changes will be discarded. In order to ensure that this is not accidentally selected a Warning will appear giving you the option to verify you want to discard your changes. This warning can be bypassed by holding down the Shift key while pressing Discard.

OK

Clicking will accept all the changes made to the model within the sculpting session and exit the form updating the Component Tree with the newly sculpted model.

Cancel

Clicking will exit the sculpting and discard ALL the changes you made within that sculpting session. The changes will be discarded even if you have previously hit Keep. If you wanted to keep most of your changes but discard just the ones you made since the last Keep then you should hit first then . In order to ensure that this is not accidentally selected a Warning will appear giving you the option to verify you want to exit and discard ALL your changes. This warning can be bypassed by holding down the Shift key while pressing .

Modeling | Slice Model

The slicing feature allows the user to divide the Composite Model into Z-Slices each of which will become a Component. This is for customers who need to cut a part which exceeds the Z depth of their machine gantry, the cutting length of their tools or the thickness of the material they are using. Once the slices have been cut on the CNC then they can be re-assembled to make the finished full depth part.

When this function is executed each slice will become a Component in the Component Tree and can then be moved into position and have toolpaths calculated on it. An example of this is shown in the images below, on the left it shows a scallop shell component that is 3 inches thick, the image below right shows this divided into two separate components, each a 1.5 inch slice of the original.

Before slicing
After slicing

Note

Before using the Slice model command it is important to make sure that you hide any components that you do not wish to include in the operation.

When the icon is clicked the Slice Model form will appear. This can be used to control the number and thickness of slices which will be created. At the top of the form it will display some reference information showing the thickness of the current Composite Model and also the currently defined Material Thickness (for machining).

Model Slicing

Slice Thickness

Checking ✓ this option will let you define a particular value for each slice. Right below this the Number of Slices will be displayed which is determined by the Composite Model thickness divided by the Slice Thickness. The model will be sliced from the bottom up and if the Composite Model thickness does not divide exactly by the Slice Thickness then the top slice may not be a whole number. To help indicate how the part is going to be divided the Top Slice Thickness is displayed in the form.

Example

If the Composite Model is 4.75 inches thick and you define a Slice Thickness of 2 inches then the software will create 3 Component slices - the bottom and middle slice will both be 2 inches thick and the top slice will be 0.75 inches thick.

Number of Slices

Checking ✓ this option will divide the model into a specific number of slices. The slice thickness will be determined by the Composite Model thickness divided by the Number of Slices defined. This may be a good option to use if the specific slice thickness is not important (for instance if it does not relate to material thickness).

Example

If the Composite Model is 3.96 inches thick and you define 3 Slices then the software will create 3 Component slices each 1.32 inches thick.

Create Boundary Vectors

Checking ✓ this option will cause the slicer to create vector boundaries for each slice. These can be useful for defining the subsequent machining regions required to cut each part. The boundary vectors will be placed on the same layer in the 2D View as the component preview for their associated model slice.

Slice Model

Clicking will apply the choices made in the form and create the Components which represent each slice of the Composite Model.

Note

The Component Tree will retain a copy of the original Components in the part as well as the new Slice Components. This may result in a very thick looking model as all the slices will be added to the original shapes. At this point you can delete, undraw or move Components before proceeding with any additional operations.

Close

Clicking will close the Slice Model form without completing the operation.

Modeling | Smooth Components

Often it is advantageous to apply a general smoothing effect over the whole of a component (rather than smooth a particular area with the Sculpting Tools). To use this tool, select the components you wish to smooth and then click the Apply smoothing filter to selected components icon on the Modeling tab. The form will appear and Cut2D Pro will take a few seconds to prepare the model for the smoothing operation. You will see a progress bar at the bottom of the screen while it is doing this.

One or more Components can be selected for Smoothing. If you select multiple shapes or a Component Group then the software will need to Bake your selection into a single Component, if applicable you should ensure you have a safe copy of your current Components before proceeding.

If you wish to smooth individual components one after another, potentially with different amounts of smoothing, you can do this by selecting one component, apply a suitable smooth filter value with the slider and then hit the Bake Current Smoothing button in the form and then proceed to selecting the next component you wish to smooth. When pick a new Component the software may take a few seconds to pick it and apply the smoothing filter to it at the default of 50% strength. If you do not click on the button before you select a new component then the effects of the smoothing will be lost on the previously selected component.

Note

Smoothing should be performed with both the 2D and 3D View visible (Tile Windows), so you can easily see the selected Component in the 2D View and also view the effects of the smoothing in real time on the 3D model in the 3D View.

Smoothing

This slider will allow the user to control the strength of the smoothing applied to the Component. By default 50% smoothing is applied, using the slider different levels of smoothing can be applied to the model. Find the strength which gives you the amount of smoothing you require. If the Max setting has not smoothed the model enough then hit the Bake Current Smoothing button which resets the smoothing slider to allow you to do further smoothing.

Preserve Transparency

Checking ✓ this option will keep the smoothing only on the current 3D areas of the selected shapes and not smooth the edges into the background. Un-checking this option will smooth all the edges of the modeled area into the background of the part, blurring the silhouette of the Component.

Bake Current Smoothing

The button bakes the current smoothing value into the Component and resets the form. This means you are able to perform multiple smoothing operations without leaving the function.

Modeling | Turn and Spin

The Turn and Spin tool allows you to create a 3D component by turning or spinning a cross section (an open vector)

Turn

Turn takes a profile and turns (rotates) it around line from start point to end point to create a rounded symmetrical shape. To turn a shape select the vector cross section you want to turn and use the Turn (Rotate) option, this cross section should represent the silhouette of the shape you wish to create. You can click to create your 3D turned shape.

[object Object]
Vector Cross Section to Turn around line from Start Point to End Point
[object Object]
Result of Turned Shape in 3D View

The profile to be turned can run beneath the line between the two end points

[object Object]
Vector Cross Section to Turn (Blue) around line from Start Point to End Point (Red)
[object Object]
Result of Turned Shape in 3D View

Spin

Spin takes a profile and spins it around the left end point of the cross section to create a circular component based on the profile shape of your cross section. To spin a shape select the vector cross section you want to spin around the left end point and click to create your 3D spun shape.

[object Object]
Vector Cross Section to Spin around Left End Point
[object Object]
Result of Spun Shape in 3D View

Note

The Spin Tool will always Spin around the left end point, which may require you to move your vector to the right side of your job to accommodate the vector being spun to create the spun shape.

Scale to Exact Height

Checking ✓ this option scales the shape calculated so its maximum height is the value entered in the Height area of the form.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Modeling | Two Rail Sweep

Two Rail Sweep uses a combination of vectors to define a swept 3D Component. The shape is based on two drive rails which can be open or closed vectors and multiple cross sections which are positioned on the drive rails and have to be created using open vectors.

Drive Rail Selection

The first stage of using this tool is to select the vectors which will represent the Drive Rails. From the 2D View use the mouse to select two open or closed vectors then click the button.

In the 2D view your rail vectors will now be colored red (first selected vector) and green (second selected vectors) and show a square green start node indicating the start point of each rail and arrow markers along its length to show the direction the shape will be swept.

The start point and direction may not be what you intended. To change the direction, right-click with the cursor on the drive rail you want to edit and select from the context sensitive menu, you will now see the arrows on the drive rail change direction.

You can also change the order the rails were selected by clicking on this will swap so the red rail becomes green and green becomes red, doing this will cause the cross-sections to hang in the opposite direction. On a closed vector you can change the start point by placing the cursor over an existing node in the drive-rail vector, right-clicking and selecting or you can right-click anywhere on the vector and select Insert Start Point to create a new node which will become the start point.

The button on the form can be used at any time to empty your current selection. This will delete your current shape and deselect all the drive rails and cross section vectors. This can be used if you do not want to create a Component before you exit the form or if you want to select new vectors in the 2D view to use as the drive rail for your shape.

Cross Section Selection

After you have chosen your drive rails the next step is to select one or more cross-section vectors to sweep along those vectors to form a 3D shape. In order for vectors to be used as valid cross-section shapes, they must be open.

Select a vector that you wish to use as a cross-section in the 2D View by left clicking on it with the mouse.

If you are using just a single cross section then you just need to make sure it is selected and then can proceed with the other settings in the form and calculate your shape. If you want to edit cross section positions or add more than one cross section then you will need to attach them to the drive rails.

Select a vector that you wish to use as a cross-section in the 2D View by left clicking on it with the mouse. Now click on the drive rail to attach the cross-section to that vector.

As you move the mouse over a selected drive rail it will indicate with a check mark ✓ that it is a valid place to add the cross section. Once a cross-section has been successfully attached to your drive rail, the 2D view will show a preview using line markers to indicate how the cross section will be positioned when it is extruded.

Two Cross-Sections are always created when you attach the first cross-section to the drive rail - one across the start nodes of each vector and one across the ends. The intermediate lines along the entire length of the rails indicate how the shape will flow between the defined cross sections. You can click the button to create your 3D swept shape.

[object Object]
Adding Cross Sections
[object Object]
Result From Two Rail Sweep

Using multiple cross-sections

It is possible to extrude between multiple cross section vectors along a drive rail blending from one vector shape to another.

Adding Cross-Sections

To add a new Cross-Section to an existing extrusion, simply select an open vector in the 2D View that you wish to use as a cross-section. With the vector selected, click on the point along the rail to which you wish it to be attached. A new Cross-Section will be inserted at this point and automatically attached to the second rail. On applying the change, the resulting 3D sweep will blend between all the defined Cross-Sections along the rail.

Adding Cross Sections
Adding Cross Sections
Result From Two Rail Sweep
Result From Two Rail Sweep

Note

To help differentiate which cross section is being used at each location the software will indicate a colored node at one end of each cross section and place the same colored node on the preview position. This node also indicates the direction the cross section is being 'hung' across the rails. The same cross section vector can be used in multiple locations along the drive rail.

Connecting Rail Nodes

By default, Aspire sweeps the cross-section along the drive rails connecting points at the same proportional distance along each rail's length. So, for example, the positions halfway or three-quarters of the way along each drive rail will be connected by the cross section in the resulting 3D shape.

As the images above show, when the matching proportional positions along each rail do not match the appropriate features of the shape it can produce undesirable results. In this example the corners of the frame design are at different proportional positions along each rail and so the two-rail sweep does not connect the corners. Instead the cross-section appears stretched around the frame, as it is used to connect other points that do match in their proportional distance along each rail.

To resolve this, the software allows you to force the connection of pairs of points along the drive rails. This can either be done manually by inserting and re-positioning the cross-sections across the corners (see sections below for more information on this), or if both the drive rails have the same number of nodes it can be done automatically after you have added the first cross section by right-clicking on the first cross section preview position and selecting Add To All Rail Nodes. This will add that same cross section to every pair of nodes on each drive rail. When the cross section positions are set up correctly then Aspire will sweep the shape between each cross section location and create clean corners as shown in the images below.

Removing Cross-Sections

To remove a Cross-Section, position the cursor over the cross section and press the RIGHT button on the mouse. Select the option to Delete Cross Section from the menu.

You can remove all the Cross-Sections on the drive rails by positioning the mouse arrow over a part of the curve that does not contain a cross section. This will bring up a different context sensitive menu and you can select the options to Remove All Cross Sections.

Altering Existing Cross-Sections

Existing cross-sections can be re-positioned on the drive rail. To do this click on the nodes at either end of the cross section preview in the 2D View (the ones on the rails), hold the mouse down and drag the node to a new position on the curve, let go of the mouse button to release that end of the cross section in its new position. You should make sure you do not drag a cross section past another existing cross section on the shape. If you need to move cross sections out of their current order then you should remove the existing cross section and insert the same shape at the new position so the shape can be created correctly. Any of your current cross-sections can be replaced by selecting a different open vector, moving the mouse over the end node of the cross section you want to change and clicking on it. The node color indicated on the cross section preview position on the curve will change to indicate which vector is now being used at that point in the shape.

Controlling the Swept Shape

There are check boxes in the form that allow you to Scale cross sections with width, Sweep between spans, and Fill center of inner closed vector rails. The Smooth option under the right-click menu allows you to control different aspects of the shape you create with the selected set of vectors.

Scale cross sections with width

As the cross sections are extruded along the rails the user can either choose to retain the exact shape and height of the cross sections or for a more natural look the Scale cross sections with width option can be checked ✓. This will alter the height of the cross section in proportion to the distance between the rails. This means that as the rails get further apart the shape gets higher and as they get closer together the shape gets lower. The image below left shows the result if this option is un-checked and below right with it checked ✓.

Scale cross section with width un-checked
Scale cross section with width un-checked
Scale cross section with width checked ✓
Scale cross section with width checked ✓

Sweep between spans

This option only becomes active if all selected cross section vectors have the same number of spans and nodes. When checked ✓ it will ensure that as the shape is extruded that it goes from a particular node/span in one cross section to the same node/span on the next cross section. In certain shapes this can give the user more control over the way the shape flows.

Sweep between spans checked ✓
Sweep between spans checked ✓
Sweep between spans un-checked
Sweep between spans un-checked

Fill center of inner closed vector rails

If you are sweeping two closed vectors to form a border or boundary shape, you can have Aspire automatically find the height that the cross-section forms on the inner boundary and then fill the shape to this height. To activate this check ✓ the Fill center of inner closed vector rails option in the form. This tool is perfect for sweep decorative bases, plaques or stands. Below left you can see a shape created with this option off and on the right an option with it activated.

Fill center un-checked
Fill center un-checked
Fill center checked ✓
Fill center checked ✓

Smooth transition through the Cross Sections

As the swept shape passes through each cross section the default is for it to flow smoothly through the profile. This can be edited by right-clicking over the end node of the cross-section and unchecking the Smooth option.

Smooth checked ✓ on all cross sections
Smooth checked ✓ on all cross sections
Smooth un-checked on all cross sections
Smooth un-checked on all cross sections

Scale to Exact Height

Checking ✓ this option scales the shape calculated so its maximum height is the value entered in the Height area of the form.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Toolpaths | 2D Profile Toolpath

Profile Machining is used to cut around or along a vector. Options provide the flexibility for cutting shapes out with optional Tabs / bridges plus an Allowance over/undercut to ensure perfect edge .

Profile toolpaths can be outside, inside or on the selected vectors, automatically compensating for the tool diameter and angle for the chosen cut depth.

When working with open vectors the profile toolpaths can be to the Left, to the Right or On the selected vectors.

Clicking this icon opens the 2D Profile Toolpath form which is shown at the right; the functions in this form are described on the following pages.

If you have vectors which are nested (like the letter 'O'), the program will automatically determine the nesting and cut the correct side of the inner and outer vectors. In addition, the program will always cut the inner vectors before the outer vectors to ensure the part remains attached to the original material as long as possible.

Design Scaling

When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click .

Job Size

This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).

It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).

Pass Depth Control

When a toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description) is used to determine the number of passes needed to profile down to the specified Cut Depth. However, by default the software will also modify the precise step down by up to 15% in either direction, if by doing so it is able to total number of passes required to reach the desired cut depth. It is nearly always desirable to benefit from the significantly reduced machining time of cutting using less passes if possible. Nevertheless, there are some occasions where the exact step down for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section page indicates how many passes will be created with the current settings.Thebutton will open a new dialog that enables the specific number and height of passes to be set directly.

Specify Pass Depths

The Pass Depths section at the top of the form shows a list of the current pass depths. The relative spacing of the passes is indicated in the diagram next to the list. Left click on a depth value in the list, or a depth line on the diagram, to select it. The currently selected pass is highlighted in red on the diagram.

To edit the depth of the selected pass, change the value in the Depth edit box and click .

The button will delete the selected pass.

The Passes button will delete all the passes.

To add a new pass, double left click at the approximate location in the passes diagram that you wish to add the pass. A new pass will be added and automatically selected. Edit the precise Depth value if required and then click .

The Set Last Pass Thickness option will enable an edit box where you can specify the last pass in terms of the remaining thickness of material you wish to cut with the last pass (instead of in terms of its depth). This is often a more intuitive way to specify this value.

Pass Depth List Utilities

This section of the form includes two methods for creating a set of passes in one go.

The first method simply sets the passes according to the Pass Depth property of the selected tool. By default, this is the method used by Aspire when it creates profile passes initially. However, the Maintain exact tool pass depth option checked, ✓ the software will not vary the step size to try and optimize the number of passes (see above).

The second method creates evenly spaced passes according to the value entered in the Number Of Passes edit box.

To apply either method click the associated button to create the resulting set of pass depths in the passes list and diagram.

Note

Setting the number of passes with either of these utilities will discard any custom passes you may have added.

Machine Vectors...

There are 3 options to choose from to determine how the tool is positioned relative to the selected vectors.

Outside

[object Object]
Calculates a profile toolpath around the Outside of the selected vectors, with options for the cut direction to be either,

Inside

[object Object]
Calculates a profile toolpath around the Inside of the selected vectors, with options for the cut direction to be either; Climb (CCW) cutting direction or Conventional (CW) cutting direction

On

[object Object]
Calculates a profile toolpath around the On the selected vectors, with options for the cut direction to be either, Climb (CW) cutting direction or Conventional (CCW) cutting direction

Direction

Can be set to either Conventional or Climb machining where the cutting direction depends upon the strategy selected - see above for details. Using Climb or Conventional cutting will largely be dictated by the material is being machined and the tooling.

Allowance offset

An Allowance can be specified to either Overcut (negative number will cut smaller) or Undercut (positive numbers will cut larger) the selected shape. If the Allowance = 0 then the toolpaths will machine to the exact size.

Do Separate Last Pass

A separate allowance can be specified for the last pass. If this allowance is given then all but the last pass will be undercut by the specified allowance with the final pass being the only pass which cuts to size.

Note

This is intended to be just a thin skin of material to be cut away as the tool will have to cut through this allowance at the full depth of the cut where all the previous passes undercut. There will be a warning displayed if the last pass allowance is greater than 1/3rd of the tool diameter but the last pass allowance should ideally be kept a lot smaller than this. Keeping this as small as possible reduces the chances the final pass will fit in areas where the previous passes will not and reduces the amount of material the last pass is having to cut through. If using a last pass allowance for the toolpath you should check that you are happy with the amount of material left for the last pass to cut through. The toolpath will fail to calculate if the last pass is cutting a significant distance into material which has not been cleared by the previous passes.

[object Object]
The final pass (shown in blue) cuts to size. All previous passes (shown in red) are cut with a small allowance offset

If the Reverse direction button is checked ✓ then the cutting direction of the last pass is reversed. This feature is can be useful if for minimizing witness marks on the edge of profile cuts.

The last pass allowance will also take into account any allowance offset and so the two options can be used together.

[object Object]
The last pass allowance will respect any allowance offset also specified


Use Vector Start Point

Use Start Point can be selected to force the toolpath to plunge and start cutting at the first point on the shape. This is very useful if you need to ensure the cutter doesn't plunge onto a critical part of the job. For example, setting the Start Point to be on a corner will often be the best position to plunge and cut from as this will not leave a witness / dwell mark on the machined surface.

The Start Points are displayed as Green boxes on all vectors when this option is selected. Start Point on a vector can be moved using the Node Editing Tools. Select Node Editing cursor or press N. Place the cursor over the node to be used as the Start Point. Click Right mouse button and select Make Start Point (or press P) Remember, you can also insert a new point anywhere on a vector using the Right mouse menu or pressing the letter P - this will insert a new point and make it the start point.

Note

Selecting Use Start Point may result in less efficient toolpaths (increased cutting times) because it may take the machine longer to move between each shape being cut. If this option is not selected the software will try to calculate the shortest toolpath, minimizing the distance between link up moves. But the downside is that the cutter may plunge/mark important surfaces on the machined edge.

Tabs (Bridges)

Tabs are added to open and closed vector shapes to hold parts in place when cutting them out of material.

Add tabs to toolpath

Checking ✓ the Add tabs option will activate tab creation for this toolpath. The Length and Thickness specify the size of each tab. Checking ✓ the Create 3D Tabs option will create 3D Tabs, the difference between this and 2D Tabs is described below.

Create 3D Tabs

When this option is selected the tab will be triangular in section. This is shape is created as the cutter ramps up to the specified Tab Thickness then down the other side. The 3D Tabs will often allow the machine to run quicker and smoother because it does not have to stop to move in Z at the start and end of each tab.

3D Tab

If this option is unchecked, the 2D tabs will be used. The cutter stops at the start point for each tab, lifts vertically by the specified Thickness runs across the ramp, stops and plunges down the other side.

How the lenght and thickness change the tab size

Profile Options

The Profiling options section of the toolpath form contains five additional pages, each of which allows a particular set of Profile machining options to be specified. The precise number of option pages will depend on which Toolpath strategy you are currently using. The full range of option pages are:

  • Ramps
  • Leads
  • Order
  • Start At
  • Corners

These help control ways to ensure the parts are held in place and machined as easily as possible while ensuring the highest quality edge finish.

Each set of options can be accessed by the tabs at the top of the Profile options section.

Ramp

Ramp moves are used to prevent the cutter from plunging vertically into the material. The cutter gradually cuts at an angle dropping into the material significantly reducing cutter wear, heat build-up and also the load on the router spindle and Z axis of the machine. If multiple passes are required due to the Pass Depth being less than the Cut Depth, the ramp moves are applied at the start of each level. All ramp moves are performed at the plunge rate selected for the current tool.

Smooth

This option creates a smooth ramp into the material using either the specified Distance or Angle.

When a Lead In distance has been specified, the option Ramp on Lead In disables the distance and angle options and automatically limits the ramp moves to only be on the lead in portion of the toolpath.

Zig Zag

This option ramps into the material by Zig-Zag backwards and forwards using either the specified Distance or Angle and Distance.

The Distance option ramps into the material, zigging for the specified distance in one direction then zagging back over the same distance.

The Angle option is typically used for cutters that cannot plunge vertically but have an entry angle specified by the manufacturer.

Spiral

Checking ✓ this creates a continual spiral ramp, these are only available when the toolpath does not include lead in moves.

This option ramps into the material over the complete circumference of the profile pass. The angle is automatically calculated to ramp from the start point to full depth over the perimeter distance around the job.

The rate at which the cutter ramps into the material is determined by the Pass Depth specified for the cutter. For example, Spiral Profiling 0.5 inch deep with a cutter that has a Pass depth of 0.5 or greater will spiral down in 1 pass. Editing the Pass depth to be 0.25 inch results in the 2 spiral passes around the profile.

Leads

Lead in / out moves can be added to profile toolpaths to help preventing marking the edges of components with dwell marks that are typically created when a cutter is plunged vertically on the edge of the job.

Straight Line Lead

This option creates a linear lead onto the cutter path using the Angle and Lead length distance specified.

The toolpath will lead onto the selected edge at the specified Angle.

Checking ✓ the Do lead out option results in an exit lead being added at the end of the toolpath off the machined edge.

The Overcut Distance forces the cutter to machine past the start point and is often used to help produce a better edge quality on parts.

Circular Lead

This option creates an arc lead onto the toolpath using the Radius and Lead length distance specified.

The toolpath will curve onto the selected edge, tangent to the direction of the vector at the point it reaches the actual geometry edge.

Checking ✓ the Do lead out option results in an exit lead being added at the end of the toolpath off the machined edge.

The Overcut Distance forces the cutter to machine past the start point and is often used to help produce a better edge quality on parts.

Order

The order tab allows you to specify the approaches the program will use to determine the best order to cut your vectors. You can specify multiple options, in which case the program will calculate the result of using each option and select the one which results in the shortest machining time.

Vector Selection Order

This option will machine the vectors in the order in which you selected them. If you have vectors inside each other (like in the letter 'O'), the inner vector will always be machined before the outer one regardless of the selection order.

Left to Right

This option will join up parts on the left of the material first and move across to the right.

Bottom to Top

This option will join up parts on the bottom of the material first and move up to the top.

Grid

This option will join use a grid based approach with the size of the grid based on the size of the parts. The algorithm will try to join up parts within a particular section of the grid before moving on.

Shortest Path

This option use a 'shortest path' algorithm to try and determine the shortest possible path. However, for large numbers of parts this requires an unfeasible amount of computing power so an approximation algorithm is used. Although very good, this algorithm cannot guarantee to produce the very shortest path, but in tests at Vectric, the results have been very good indeed. This option still takes a substantial amount of time on slow computers of for very large numbers of parts.

Start At

Keep Current Start Points

The start point of the vector will dictate the start of the toolpath.

Optimize Start Points

The software will automatically attempt to optimize each profile start position based on speed of completing the job.

Closest on Bounding Box

Influence the start point by defining which part of the bounding box of the profiled vector it should start near.

This will look for the nearest point, from all of the spans' endpoints, and will start the toolpath from that point.

Corners

Choosing this tab and checking ✓ the option Sharp external corners (see below) forces the cutter to machine around the shapes and retain any square corners.

Sharp External Corners

This option makes adding beveled edges to a 2D shape very quick and easy, this can be a good way to turn simple 2D cut out lettering into a high quality signage products that look more interesting or provide a different option for customers.

This is an example of the type of effect that can be created by using this option:

Standard Profile toolpaths without the Sharp Corners switched on roll around the sharp corners. This Still give a point on a straight sided tool but will give a radiused edge when using a V-bit.

When Sharp External Corners is selected the following change is made to the toolpath (see image below) so it makes sharp external corners as shown in the image of the letter 'M' at the top of the page.

Sharp Internal Corners

When Sharp Internal Corners is selected the V-Bit tool will raise up into internal corners to sharpen them with its point. The difference between checking ✓ this and leaving it unchecked is shown in the two images below.

Sharp Internal Corners not selected
Sharp Internal Corners not selected
Sharp internal corners selected
Sharp internal corners selected

Allowance for Cut out tool

Sharp internal corners are often used when creating beveled letters. In this case, the letters usually have straight 'returns' which are machined with a straight sided end mill. The cut out pass for the end mill needs to be offset from the vector to allow for the bevel created by the tool. This field displays the value you will need to enter into the 'Allowance Offset' field when you create your cut out profile toolpath for the end mill. You can select the value with the mouse and used Ctr+C to copy it to the clipboard and then copy it into the 'Allowance Offset' field when you create the cut out toolpath.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | 3D Finish Toolpath

Finish Machining is used to machine the final pass on the finished 3D part.

For most 3D Finishing cuts a Ball Nosed end mill is used with a reasonably small stepover (8 - 12% of the tool diameter is typical). Variations on this tool type such as a tapered Ball Nosed cutter will also work and may offer more strength with smaller tool sizes. The size of tool will depend on the size of the part and the detail within the 3D part. Use the preview function to check the finish quality and detail; if they are not to a high enough standard then the job may require smaller tooling or a smaller stepover. 3D cutting is always a tradeoff between time and quality and an optimum balance of tool size, finish quality, and time to cut. The choices made will always depend on an individual's personal preferences or the specifications of the job.

Note

The finishing toolpath is always a single pass, and it does not use the tool's pass depth. Please ensure that your Roughing Toolpath's Machining Allowance is set appropriately for the tool used in Finishing to avoid damaging the bit.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Boundary Offset

If you are machining a raised object, often the tool will not fully machine down the edge. This field is used to specify an offset to the selected machining boundary to increase its size to allow the tool to go past the actual edge if needed.

Note

The cutting side of the tool will not leave machining boundary.

Area Machining Strategy

There are two choices of the type of fill pattern that will be used to machine the area with the toolpath; Offset and Raster.

Offset

[object Object]

Your choice of Climb or Conventional cutting will largely be dictated by the material that is being machined and you're tooling options. Talk to your tooling suppliers for details about what is most appropriate for your specific application.

Raster

[object Object]

Calculates a raster pattern (lace cut) projected onto the 3D surface and machined inside the selected vector(s), with control over Raster Angle - Between 0 and 90°. 0° will give you a pattern that is mainly parallel to the X axis and 90° is mainly parallel to the Y axis.


Stepover Retract

The Stepover Retract Value can be applied to the Offset Machine Strategy. If the value you enter is greater than 0 then the tool will lift off the surface of the composite model by this amount when stepping between each offset contour. Depending on your material and tooling, adding a small lift will eliminate perpendicular tool marks between the toolpath contours to potentially improve the finished surface.

Note:

If the Stepover Retract Value specified is not large enough to allow the machine to lift the tool over the previous cusp height then you will receive a warning. This warning is simply informing you that with a Stepover Retract value of this size then you will not eliminate perpendicular tool marks.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | 3D Rough Toolpath

Rough Machining is used when carving 3D parts to clear away excess material when the part is too deep for the finishing tool to cut in a single pass.

Clicking on this icon opens the toolpath form shown to the right; the functions available within this are described below.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Boundary Offset

If you are machining a raised object, often the tool will not fully machine down the edge. This field is used to specify an offset to the selected machining boundary to increase its size to allow the tool to go past the actual edge if needed.

Note

The tool tip (rather than the cutting side) will not leave the machining boundary. This is to help ensure that roughing removes enough material on machining boundaries.

Machining Allowance

The machining allowance is a virtual thickness which is added to the 3D model when the Roughing Toolpath is calculated. This ensures that the toolpath leaves some extra material on the roughed part.

This is beneficial for two main reasons, the first is that when roughing it tends to be done with relatively large tool and aggressive cuts and so is more prone (depending on the material) to chip, this skin helps to prevent the chipping affect the finished surface. The second reason is that most tools cut well when they are constantly removing material. Therefore leaving an allowance of material on ensures that there is always at least some material for the finishing toolpath to remove.

Roughing Strategy

The roughing strategy determines the process the toolpath will take to remove the desired material

Z Level Strategy

Z Level Roughing essentially uses a series of 2D Pocket toolpaths which take into account the 3D model and hog-out the material around it within the specified boundary.

The first setting is the choice of Profile, this controls whether each level has a profile cut around its boundary or not and if so whether it cuts before the raster or after it. First does the profile before the Raster on each level, Last does the profile cut after the raster and None eliminates the Profile cut leaving only the raster pattern. These choices depend a lot on the material and tooling being used. For example, more brittle material may benefit from the profile first option to reduce chipping.

The second setting is the choice of Order. The Z Level can be performed in Level by level manner. This means to generate a complete pass at a given depth over the whole model, before advancing to the next level. This is the default option.

The user can also select Depth-first. In this case if at a given depth the model consists of separate regions, the generated toolpath will generate all passes at increasing depths over such region. Then it will advance to another such region.

3D Raster Strategy

The 3D Raster strategy is a 3D cut which passes over the whole model. This will leave a more even amount of material for the finish cut to remove but depending on the depth and style of the part it may take significantly longer to run. In shallower parts where the roughing is only taking one or two passes then this may be a better choice. For deeper parts then typically the Z Level rouging is a more efficient.

Raster direction

This option allows to define the main cutting direction. Along X uses a raster pattern parallel to the X axis or Along Y uses a raster pattern parallel to the Y axis.

Reverse step direction

By default, when using raster direction Along X the tool will move from one raster line to another from bottom to top. In case of raster direction Along Y the tool will move from right to left. This option allows to reverse that stepover direction.

Note

This option is currently only available for Z Level strategy.

Ramp Plunge Moves

The cutter can be ramped over a distance into the pocket instead of plunging vertically. This approach reduces heat build-up that damages the cutter and also reduces the load on the spindle and z axis bearings

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Array Copy Toolpath

Using the same approach as the Array Copy Tool for vectors in your drawing, this toolpath operation allows you to duplicate one or more toolpaths into a grid of copies. One of the key benefits of this approach is that it allows you to subsequently edit your original toolpaths and the software will automatically update the associated array of copies.

Toolpath Selection

To use the Array Copy Toolpath, open the form and turn on the visibility for each of the toolpaths you wish to be part of your array using the visibility checkbox next to each toolpath in the list below the form. The current selected toolpaths appear in the Toolpaths list at the top of the form.

The position of the resulting grid of toolpaths is always created to the right and above the source toolpaths. Therfore, you should always position your source toolpaths in the bottom left corner of the area you wish the array to fill.

Rows and Columns

Use the Rows (Y) and Columns (X) boxes to specify the size of your grid and thus the total number of copies of the original toolpath(s) that will result.

Spacing

The spacing between the copies of the toolpath within the grid are controlled using the Offset and Gap radio button options. The X and Y edit boxes determine the offset between the start point of each toolpath or the spacing between the bounding boxes of the copy, depending on the radio button option selected.

Minimize Tool Changes

The final option, Minimize tool changes, will only be available if the source toolpaths are using different tools. This will group toolpaths with the same tool geometry across the copies so that they can be output together. By grouping in this way, the parts of each copy using the same tool are cut together and the entire array can be cut with the minimum number of tool changes. If this option is not set, then the toolpaths for each copy will be cut individually, with tool changes required for each. See the The Array Copy Toolpath Cut Sequence

Working with Array Copy Toolpaths in the Toolpath List

Array Copy Toolpaths are displayed in the Toolpath List in different way to other toolpaths. The source toolpaths (the ones originally selected as the basis of the array) are now shown below the array copy toolpath item in a tree structure. For complicated jobs you can hide the source toolpaths in the list using the small and controls next to the Array Copy Toolpath in the Toolpath List. The usual visibility checkboxes are also available for both the array copy toolpath and its source toolpaths.

You can rearrange the order of the source toolpaths within the array copy group either by dragging them up or down using the mouse, or by click the up and down ordering arrows at the top of the Toolpath List. These features give you total control of each toolpath type within the array and are particularly important for saving the toolpaths

Saving an Array Copy Toolpath

As far as possible, array copy toolpaths are saved in exactly the same way as other toolpaths except that each source toolpath in the list represents all of its copies. If you switch off the visibility of a source toolpath before saving, noneof the copied instances of that toolpath will be included in the saved toolpath. Thus you can use the visibility controls to save a toolpath that will cut all of the copies, but limited to a particular subset of the source toolpath types.

In general, the sequence of cutting will be to cut all of the included toolpath strategies for each copy in the grid before moving on to the next copy.

Important

If the array copy toolpath contains more than one source toolpath using the same tool, then the sequencing within the array copy toolpath as a whole can be affected by the Minimize tool changes option setting when it was first created.

Minimize

Toolpaths | Create Job Sheet

Job sheets contain a summary of the information you will need when you come to run the toolpaths for your project at your CNC machine. Aspire will create a self-contained HTML document that can be viewed using most web browsers, including Internet Explorer, Chrome or Firefox. To create a job sheet for a given project, simply select Create Job Sheet from the Toolpaths menu and then select a filename and location to save the document. If your job contains multiple sheets, Aspire will automatically create a Job Sheet for every sheet that contains toolpaths. If you are working on a two sided job you will need to create a job sheet for both sides by simply switching between the sides and selecting the create job sheet icon, when you save the .html file the software will automatically add “_Top” or “_Bottom” to the name to differentiate between the two sides once the file has been saved.

Auto Open

If you wish to automatically open the Job Sheet after creation, simply hold down the CTRL key on the keyboard as you select the Create Job Sheet option from the menu.

Each job sheet document comprises the following information:

Job Layout

A thumbnail image representing the vectors on your current job / sheet, surrounded by an outer rectangle representing your material size.

Material Setup

A summary of the important pieces of information you will need to correctly position and datum your work piece at your CNC machine. This includes the dimensions of the material block used within Aspire to create and simulate your toolpaths. The home position from which your machine will start and return to. The clearance above the material for any rapid moves between plunges. For Two Sided Jobs you will also be displayed which side the setup sheet belongs to (top or bottom) along with the flip direction.

Toolpaths Summary

A summary of each of the toolpaths in the file, including the name of the toolpath, the tool required and an estimate of how long it will take to cut.

Toolpaths List

Details of each toolpath, including feed and plunge rates plus the intended spindle speed.

Toolpaths | Delete Toolpath

This tool is used to delete calculated toolpaths from the Toolpath List. Simply select the toolpath to be deleted and click the Delete Toolpath button to remove it.

Alternatively, you can delete one or multiple toolpaths in the Toolpath List by right mouse clicking on a toolpath. Then from the drop-down menu click on the Delete option. This will present the options as shown in the image: Delete This, Delete All Invisible, Delete All Visible, Delete All.

Delete This will delete just the toolpath whose name you right mouse clicked on.

Delete All Invisible will delete any toolpaths in your Toolpath List that do not have a check-mark ✓ next to their name and are therefore currently not visible in the 2D or 3D Views.

Delete All Visible will delete any toolpaths in your Toolpath List that have a check-mark ✓ next to their name and are therefore currently visible in the 2D or 3D Views.

Delete All will delete all the toolpaths in your Toolpath List.

If you have incorrectly deleted a toolpath (or multiple toolpaths) then you have the option to Undo the toolpath(s) deletion via the Undo command on the Edit drop-down menu, the Undo icon on the Drawing Tab or the Undo shortcut key combination Ctrl + Z.

Toolpaths | Drilling Toolpaths

Drilling allows the centers of selected closed vectors to be drilled to a specified depth. The Tool Database includes an option to specify the Drill diameter and cutting parameters.

Cutting Depths

Start Depth (D)

This specifies the depth at which the toolpath is calculated from.

When cutting directly into the surface of a job the Start Depth will often be 0. If machining into the bottom of an existing pocket or 3D region, the depth needs be entered.

Cut Depth (C)

The depth of the toolpath relative to the Start Depth.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Peck Drilling

When the option Use Peck Drilling is selected, the drill will cut to the Pass Depth set in the Tool Database for the selected Drill. It will then retract to the Retract Gap according to the retract option selected (see below), before drilling to the next depth, incremented by an additional Pass Depth. This cycle is repeated until the hole is drilled to the required depth. The retract moves are used to remove any build-up of material from the hole to help with overheating and breakage. If the Pass Depth is greater than the required Cut Depth, the hole will be drilled in a single cycle. However, if a Cut Depth of 1 inch with a Pass Depth of 0.25 inch is used the hole will be drilled in 4 cycles.

Retract above cutting start

This option will cause the tool to retract fully out of the drill hole after each peck drill plunge. This is beneficial for clearing swarf/chips completely from the drill hole during the drill cycle. With this option selected the Retract Gap value (R) is the fixed distance above the start cut depth. Thus the total retract and plunge distances for each peck drill cycle will increase as the hole deepens and this will generally result in longer machining times.

Retract above the height of the previous pass

Instead of fully retracting out of the drill hole, it is also possible to retract to a height relative to the previous cut depth. This strategy typically requires a shorter set of plunges and retracts over the course of a peck drill toolpath because they will be constant for each peck drill cycle, regardless of the drill hole depth. However, it will not necessarily clear swarf/chips completely from the drill hole. With this option selected the Retract Gap value (R) is the relative distance above the height of the previous peck drill pass.

Dwell at the bottom of each drill pass

With this option checked, ✓ the Dwell Time value is used pause the drill at the bottom of each peck drill pass before retracting. The dwell time value is measured in seconds.

Note

To make use of this feature your Post-Processor must support the Dwell section and may require updating.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Duplicate Toolpath

The Duplicate Toolpath option creates and adds a copy of the selected toolpath to the Toolpath List. An index number is automatically added to the name of the new toolpath. For example:

Cut out - 1/4 inch End Mill will create a copy with the name Cut out - 1/4 inch End Mill (1)

Copying externally generated 3D toolpaths (as, for example, from PhotoVCarve) will also create a duplicate grayscale thumbnail image in the 2D View, which can then be used to position the toolpath within your job.

Toolpaths | Edit Toolpath

This option is used to modify an existing toolpath. Click to select a toolpath in the list then click the edit option to open the form.

The vectors associated with each toolpath are automatically remembered, so editing a toolpath will automatically select the vectors in the 2D window.

Make the required changes to the toolpath parameters Click the Calculate button to update the toolpath

A toolpath can also be edited by double-clicking on its name in the toolpath list.

Toolpaths | Estimating Machining Times

This option estimates the machining times for all calculated toolpaths based on the feed rates specified for each tool. The estimates for individual toolpaths plus the overall machining time of all visible toolpaths are calculated using the user defined Rapid Rate moves and Scale Factor.

Times

The estimated machining times are displayed in Hours: Minutes: Seconds

Rapid Rate

The maximum feed rate at which the machine runs for rapid moves, typically specified using a G0 or G00 move

Scale Factor

The nature of different styles of toolpaths means that they may be simple 2D cuts or require simultaneous 3-axis moves, the more complex the toolpath then the more chance the CNC machine may not actually achieve the programmed feed rates. This can be compensated for by multiplying the times by the Scale Factor.

The scale factor in the program lets you approximate this slowdown for your machine, but it will vary depending on the type of work you are doing. Many people will use one scale factor for simple 2d work and another for 3d or VCarving. The best way to calculate it is just to take a note of estimated and actual machining times of a period of time.

For machines where the controller provides an estimated machining time, these should be more accurate as the controller can determine where the machine is accelerating / decelerating and take account of this.

Toolpaths | Fluting Toolpath

Fluting Toolpaths machine along vectors while varying the depth of the tool, creating extremely efficient machined decorative patterns.

This toolpath is similar to the option to Profile On a selected vector. The difference is the toolpath at the end of each vector can be ramped to taper the cut. This can be used for cutting standard woodworking Flutes or can be used for artistic engraving and marking effects with other types of artwork. In this section the options on the form will be covered along with some examples of the use for different applications.

Selecting Vectors

When the Fluting Toolpath form is open, the selected vectors will have their start points indicated in the 2D View by solid square green nodes, this is important as it will determine which end the ramps are added depending on what options are chosen on the form. An image of this is shown below where all the start points are to the left end of the selected vectors.

If you need to move the start points, go into node editing mode (press N on the keyboard or select the node editing icon in the Edit Vectors section on the left tab).

Select the vector you want to change the start point Move the cursor over the end you want to be the new start point Press P on the keyboard or Right Click and select Make Start Point from the pop-up menu. Exit node edit mode (press N again) Reselect all the vectors you want to flute

Cutting Depths

Start Depth (D)

This specifies the depth at which the Fluting toolpath is calculated. When cutting directly into the surface of a job the Start Depth will usually be 0. If machining into the bottom of an existing pocket or stepped region, the depth of the pocket/step that you are starting from must be entered.

Flute Depth

This is the depth of the Fluting toolpath relative to the Start Depth; the total depth will be the combination of the Start and Flute Depth.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Flute Type

Ramp over complete length

Checking ✓ this option means the tool will ramp over the whole length of the toolpath. At the start of the selected vector/s it will be at the Start Depth and at the end of the selected vector/s it will have cut down to the Fluting Depth.

Ramp at Start

Checking ✓ this option means the tool will ramp down only at the start of the vectors to the Fluting Depth. The distance of this ramp can be specified using the Ramp Length or Ramp % options.

Ramp at Start and End

Checking ✓ this option means the tool will ramp down at the start of the vectors then will ramp up again at the end of the vectors. The distance of these ramps can be specified using the Ramp Length or Ramp % options.

Ramp Length

Checking ✓ this option means that the length of the ramp can be set to an exact distance entered into the box. The ramp distance is measured from the start and the end of the vector/s depending what Flute Type you have selected. If the distance entered is greater than the possible length of the ramp then the maximum length will be used, this would be the same as choosing Ramp over complete length. When you choose Ramp at Start it is possible to specify a ramp length which is up to the length of the vector/s. When Ramp at Start and End is checked, ✓ the maximum length possible would be half way along the vector/s as after that it would start to ramp up again.

Ramp %

Checking ✓ this option means that the length of the ramp can be specified as a percentage of the maximum possible ramp length (controlled by the length of the selected vector/s and chosen Flute Type). When you use this with Ramp at Start selected then 100% would be the whole length of the selected vector/s, the ramp length would be a percentage of this distance for each one. When you use this with Ramp at Start and End then 100% would be the half length of any of the selected vector/s. The ramp length would be a percentage of this half-length. In this situation using a 50% value would give you a Ramp from the start which was ¼ of the vector length and a ramp from the end which was also ¼ of the vector length.

Ramp Type

Linear

Selecting the Linear type will create a ramp which is a diagonal line (following the vector) from the Start Depth to the Flute Depth. Below you can see a Linear Ramp Type shown from the side. This ramp is set to only ramp from the start and to go 50% of the flute length.

Smooth

Selecting the Smooth type will create a curved ramp (following the vector) from the Start Depth to the Flute Depth; this will smoothly transition from the ramp into the full depth of cut. You can see an example of this shown in the image below.

Toolpaths | Inlay Toolpath

The Inlay toolpath functionality can be used to calculate either profile or pocketing toolpaths with automatic compensation for the tool radius; this allows the cut-out parts to fit into the corresponding cavities. This is a great feature for creating decorative woodwork and is also particularly useful for sign makers for creating inlayed letters and graphics.

How Inlays Work

When using a CNC machine to cut out shapes then the tool will always leave a radius on any internal corner. When cutting holes or pockets the tool conversely leaves a radius on the external corners. If no changes are made to accommodate this then there would be no way to fit one part into the other. This is shown highlighted on the letter 'T' shown in the image below. On the left you can see the internal corners with a radius on the part being cut out (highlighted with red ovals). On the right you can see the radiused external corners on the hole (highlighted with green ovals). As you can envisage trying to slot the 'T' into the hole would not work as it is the proverbial square peg in a round hole!

Inlay with radiused inner corders
Inlay with radiused outer corners

It is not possible to avoid the added radius as it is formed by the tool size and shape. The Inlay function though, will create toolpaths which take the tool radius into account and compensate for it by rounding off the sharp corners so the resulting parts will fit together. This can be seen in the images shown below where the same letter has been cut using the Inlay toolpaths, you can see all corners (internal and external) now have the same radius so they will slot together

When creating an Inlay toolpath the radius is automatically compensated for, so it is very important to make sure you specify the same tool for both parts of any inlay (male and female). If you do not do this the Inlay will not fit together.

If creating a Pocket then the main Tool (the finish tool) not the larger (clearance) tool should be the same as the one as used for creating the Male Inlay.

Note

You must use the same tool for both parts of an inlay for the resulting parts to fit together correctly.

Male Inlay (Insert)

Straight

This option is for cutting out straight sided parts to act as the inserted piece of the inlay. It uses a variation on the Profile toolpath which will automatically round the external corners of the part to allow for the radius of the tool being used. All the standard Profile options are available in this form except there is no option to Profile Inside or On as this does not apply to this inlay type as it has to cut outside of the vector. The other standard options not available are the ability to add sharp Corners or set a Last Pass as again these would not apply to this application. The image below shows how the external corners are rounded based on the tool radius being used.

Stepped

This option is for cutting out stepped sided parts to act as the inserted piece of the inlay. This style of inlay is typically used for what are referred to as 'Push Through' letters and shapes. These are parts which are inserted from the back and use the step as a shelf to invisibly mount them to the back of a sign. As with the Straight Inlay option it uses a variation on the Profile toolpath with the addition of the ability to specify a Step Depth and Step Width.

As the diagram shows in the form, the Step Depth is the vertical height of the step from the Start Depth down, the Step Width is how far from the edge of the original vector the part will be cut out (creating the step).

Female Inlay (Pocket / Hole)

Pocket

This option is selected for cutting out a Pocket to act as the cavity for the corresponding Male shape to inlay into. It uses the same options as the standard Pocket style toolpath including the new option where you can use a larger and smaller tool to clear the pocket (smaller tool size should match that used for the Male Inlay). In order to make it work as an inlay pocket any internal corners will be rounded based on the tool radius to allow the male parts to fit into them (shown in the image below).

[object Object]

As has been previously discussed it is common to leave an allowance on one or both sides of the inlay, typically when working with letters the allowance would be left on the Pocket so the size and shape of the lettering itself is not affected any more than necessary.

Hole

This option is for cutting out a Hole to act as the cavity for the corresponding Male shape to inlay through. The standard Profile options are available for Female Hole Inlays except there is no option to Profile Outside or On as this does not apply to this toolpath type and this option does not allow the use of the Corner options as these are also inapplicable to this type of toolpath. In order to make it work as an inlay, any internal corners will be rounded based on the tool radius to allow the male parts to fit into them (shown in the image below).


Toolpaths | Laser Cut And Fill

Laser Cut - Fill is used for cutting out shapes or marking areas.

Cut-outs can take into account the kerf, or width, of the laser beam to maintain the precise internal or external size the selected vector shapes. Shapes can also be filled with stripes or hatching to create simple shading effects.

Tool Selection

Select Tool

This button opens your database of previously stored laser settings for different jobs and materials. When a setting is selected fromt the database it will be used to populate the key fields in this section. You can subsequenlty modify these values when calculating the laser toolpath. Modifying the settings on this form will not alter the original stored settings within your database.

Power

This value sets what proportion of your machines maximum laser power will be used for this toolpath.

Move Speed

This specifies the maximum speed that your machine will move during cutting or engraving moves. The units are determined by the database setting that was originally selected.

No. Passes

The machine can repeat a toolpath a number of times to cut through thicker material. This value sets the number of repeats.

Strategy

Based on the selected vector shapes in your drawing, this toolpath offers four distinct strategies

Cut Outside / Right

Selecting this option will run the laser around the outside of your selected vector shapes (or along their right-hand edge, if they are open vectors). The actual path of the laser is automatically offset from the orginal shape according to the kerf width of the laser. As a result, the external dimensions of the resulting physical part precisely match the size of the original vector drawing. This strategy should be used for cutting out shapes to precisely the correct dimensions.

Cut Inside / Left

This option will run the laser around the inside (or left-hand edge) of your selected vector shapes, allowing for the kerf of the laser. This strategy is typically used for cutting holes, slots or sockets where the remaining recess has precisely the same dimensions as the original selected vector drawing.

Cut On

This option will runs the center of the laser beam along the selected vector. No offsetting or kerf compensation is required.

Hatch Fill

This is a marking or 'shading' strategy which profiles along the selected vectors and then fills-in the shapes with stripes. When this option is selected the additional Stepover, Hatch Angle and Cross Hatch options will also become enabled - see below for more information on these.

Allowance

This setting allows you to add an additional offset for the Cut Outside, Cut Inside strategies without adjusting the laser kerf settings and can be useful for easing or tightening the fit of shapes resulting from these cuts.

Note

This option is not applicable to the Cut On or Hatch Fill strategies and will be disabled if they are selected.

Stepover

When creating hatch fills, this option determines the spacing between the hatch lines. It is only available when the Hatch Fill strategy is selected.

Hatch Angle

When the Hatch Fill strategy is selected, this option determines the angle of the hatching lines used.

Cross Hatch

Checking this option will create a cross hatch fill instead of a single set of lines.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Immediate Output

Once calculated, your toolpath is stored in the central Toolpath Tree and can be saved, edited or output to your machine at anytime using the command. In addition though, this form also includes a convenient Immediate Output section that allows you to save or send the most recently calculated toolpath directly from this form without having to close it.

Post Processor

Use this drop-down list to select the post-processor for your machine.

Add side to toolpath name

If you are creating aligned toolpaths for a two-sided part, this option automatically adds the side name to the toolpath name as it is saved or exported to help keep your toolpaths organised.

Output direct to machine

If your post-processor supports direct access to your cnc machine (including machines supported by VTransfer), this option will be available. Selecting this option will bypass saving the toolpath to disk and instead send it straight to the direct output driver.

Toolpaths | Laser Picture

The Laser Picture toolpath uses the laser to etch a copy of the selected bitmap picture into the surface of your material.

Tool Selection

Select Tool

This button opens your database of previously stored laser settings for different jobs and materials. When a setting is selected fromt the database it will be used to populate the key fields in this section. You can subsequenlty modify these values when calculating the laser toolpath. Modifying the settings on this form will not alter the original stored settings within your database.

Power

This value sets what proportion of your machines maximum laser power will be used for this toolpath.

Move Speed

This specifies the maximum speed that your machine will move during cutting or engraving moves. The units are determined by the database setting that was originally selected.

No. Passes

The machine can repeat a toolpath a number of times to cut through thicker material. This value sets the number of repeats.

Strategy Settings

Raster

Selecting this option will generate a single set of parallel lines, or stripes, across your selected image.

Hatch

This option will create two sets of parallel lines at 90 degrees from one another. This strategy will generally produce a denser image reproduction, but will typcially take twice as long to etch.

Selected

This option will use the selected vectors as the pattern for the toolpath moves. These may be generated using any method of creating vectors, such as the Vector Texture Tool

Dither Image

With this option un-checked, laser power will be changed evenly in response to the lighter and darker areas of your image. Thus your image is reproduced by a range of burnt tones onto the surface of your material using continuously varying laser power. For some materials, however, the burning process tends to produce only two tones - burnt or unburnt - rendering this graduated approach ineffective. For materials with this property an alternative strategy can be used to generate the tonal range using only black dot patterns of differing densities instead - much like old newspaper picture print. This process is called dithering and it can be enabled using this option. In general you should only use this option if the material properties prevent you from using the higher quality true grayscale method.

Line Spacing

This slider adjusts the gap between the raster stripes - tight striping produces a denser image reproduction, but will take a lot longer to etch. The maximum density is set by the Kerf of your laser beam and the most sparse setting is 30 times this value.

Line Angle

Adjust this slider to change the angle of the stripes or hatching used to etch the image. Zero degrees will produce horizontal stripes and ninety degrees, vertical.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Immediate Output

Once calculated, your toolpath is stored in the central Toolpath Tree and can be saved, edited or output to your machine at anytime using the command. In addition though, this form also includes a convenient Immediate Output section that allows you to save or send the most recently calculated toolpath directly from this form without having to close it.

Post Processor

Use this drop-down list to select the post-processor for your machine.

Add side to toolpath name

If you are creating aligned toolpaths for a two-sided part, this option automatically adds the side name to the toolpath name as it is saved or exported to help keep your toolpaths organised.

Output direct to machine

If your post-processor supports direct access to your cnc machine (including machines supported by VTransfer), this option will be available. Selecting this option will bypass saving the toolpath to disk and instead send it straight to the direct output driver.

Toolpaths | Load Toolpath Template

When you load a previously saved toolpath template (using Toolpaths ► Templates ► Load Template...) you will have an empty toolpath which can be edited by double clicking on its name in the toolpath list or selecting the Edit Toolpath icon in the Toolpaths tab. Once the toolpath form is open, the vectors to be machined can be selected and the toolpath calculated using all the saved settings.

If you load a toolpath template which has toolpaths associated with layers which don't exist in the current file, the Missing Layers for Template dialog will be displayed. It lists all the missing layers and offers you the choice of having them created automatically, deleting toolpaths associated with missing layers or just loading the toolpaths as is.

Choosing to allow the dialog to automatically create the missing layers allows a toolpath template to be used to create 'standard' layers for machining operations and load the toolpaths ready to be calculated. All you then need to do is move vectors to the appropriate layers and recalculate all the toolpaths.

Choosing the Delete all toolpaths associated with missing layers option allows you to create a single template with many toolpaths and have the ones which aren't appropriate to the current job automatically deleted.

Toolpaths | Material Setup

The Material Setup section of the Toolpaths tab provides a summary of the current material settings. Some of these values will have been initially set when the job was first created (see Job Setup for more information). When you come to creating toolpaths, it is important to review this information and ensure it is still valid and also to set the machining clearances. To access all these properties for editing, click on the button to open the Material Setup form:

Different form is displayed depending on the job type:

Toolpaths | Material Setup - Flat

Thickness

Enter the thickness of the material being machined.

XY Datum

This allows you to set the X and Y origin of the job. See the section in Job Setup form

Show detailed summary on toolpath tab

This checkbox toggles the Material Setup summary layout on the Toolpaths tab between simple and detailed views.

Side Z-Zero

Select relative to the Material Surface or relative to the Machine Bed. This is a very important setting because the tooling used on the CNC machine must be setup in the same way, ensuring the toolpaths cut to the correct depth.

If you are working in a 2 Sided job, this will set the Z Zero for your current side only,

  • The side you are setting up will be displayed in brackets e.g. (Top).
  • You can set the Z-Zero for both sides through the Job Setup form.

Model Position in Material

The thickness of your model must be less than the thickness of the material you wish to cut it from. You can position your model within the material block wherever you wish by defining the gap distance either above or below your model. You can also double left click on either of the three lines next to the slider to position the model at the top, center or bottom of the material.

Note for Two-Sided Jobs

The gaps defined here are for the entire combined models from both sides (i.e. the final result you see when two-sided view is enabled). The above / below gaps do not depend on which side you are currently on. They represent the whole 2 sided model as if viewed in the correct orientation.

Gap Above Model

This distance positions your model according to the gap between the top of your model and the top surface of the material.

Gap Below Model

Alternatively you can position your model by defining the gap between the bottom of the model and the bottom surface of the material.

Model Thickness

This field simply reports the thickness of your composite model (as built from all your currently visible components).

Scale Model Height

The button can be used to change the Z Height of the Composite 3D Model (the visible Components) if it is not an appropriate height for your material thickness. Clicking this button will open the Set Model Height form which allows you to enter a new value for the overall height of the combined Components. After you have entered a new value hit and visually check the 3D model to ensure it still looks correct. Once you have found an appropriate value that looks good you can hit the button to continue in the Material Setup form. This height scaling function is also available from the Scale z height of model icon on the modeling toolbar.

Modeling Plane Z

Once you have positioned your model, this field will tell you the new height of your modeling base plane. This is for information only, and results from the gap settings above and cannot be edited directly.

Rapid Z Gaps above Material

Clearance (Z1)

This is the height above the job at which it is safe for the cutter to move at rapid or maximum feed rate. The software will raise the bottom of the cutter to this height when it traverses the material.

Plunge (Z2)

For all toolpaths, as well as specifying a rapid clearance gap for rapid positioning moves above the workpiece, the user can also specify a much smaller gap that the tool will rapid down to during plunge moves. By default the plunge gap is set to the same value as the Clearance gap which means that there will be no rapid plunges. If you set the plunge gap to a smaller value than the Clearance gap, the tool will plunge at rapid feed rate to the specified distance above the material surface before changing to the specified plunge rate. For jobs where a large value for Clearance gap has to be specified to avoid clamps etc, this feature can save a considerable amount of machining time if there are a lot of plunge moves in the job.

Note

Some engraving machines are not able to take advantage of this feature.

Home / Start Position

This is the absolute position that the tool will start moving from and where the tool can be programmed to return to at the end of cutting the job.

Toolpaths | Material Setup - Rotary

Diameter

Enter the diameter of the material being machined.

XY Datum

This allows you to set the X and Y origin of the job. See the section in Job Setup form

Show detailed summary on toolpath tab

This checkbox toggles the Material Setup summary layout on the Toolpaths tab between simple and detailed views.

Z-Zero

Select relative to the surface of the material cylinder or its center. This is a very important setting because the Tooling used on the CNC machine must be setup in the same way, ensuring the toolpaths cut to the correct depth.

Model Position in Material

The diameter of your model must be less than the diameter of the material you wish to cut it from. You can position your model within the material block wherever you wish by defining the gap distance either outside or inside your model. You can also double left click on either of the three lines next to the slider to position the model at the top, center or bottom of the material.

Gap Outside Model

This distance positions your model according to the gap between the top of your model and the surface of the material cylinder.

Gap Inside Model

Alternatively you can position your model by defining the gap between the bottom of the model and the center of the material.

Model Thickness

This field reports the thickness of the model (as built from all the currently visible components). The model can be scaled by clicking on the button.

Modeling Plane Z

Once you have positioned your model, this field will tell you the new height of your modeling base plane. This is for information only. It results from the gap settings above and cannot be edited directly.

Rapid Z Gaps above Material

Clearance (Z1)

This is the height above the job at which it is safe for the cutter to move at rapid or maximum feed rate. The software will raise the bottom of the cutter to this height when it traverses the material.

Plunge (Z2)

For all toolpaths, as well as specifying a rapid clearance gap for rapid positioning moves above the workpiece, the user can also specify a much smaller gap that the tool will rapid down to during plunge moves. By default the plunge gap is set to the same value as the Clearance gap which means that there will be no rapid plunges. If you set the plunge gap to a smaller value than the Clearance gap, the tool will plunge at rapid feed rate to the specified distance above the material surface before changing to the specified plunge rate. For jobs where a large value for Clearance gap has to be specified to avoid clamps etc, this feature can save a considerable amount of machining time if there are a lot of plunge moves in the job.

Note

Some engraving machines are not able to take advantage of this feature.

Home / Start Position

This is the absolute position that the tool will start moving from and where the tool can be programmed to return to at the end of cutting the job.

Toolpaths | Merged Toolpath

When using the same tool for different types of toolpath (eg. Pocketing and Profiling) those toolpaths can be merged to create a single toolpath which performs the same cutting operations more efficiently.

Toolpath Selection

The toolpath merge tool will always try to merge all visible toolpaths. To toggle the visibility of the toolpaths click the corresponding check boxes for each toolpath in the toolpath list shown below the form. The toolpaths to be merged will appear in the box marked Toolpaths to be merged...

Ordering

The toolpath merge tool has a number of checkboxes which allow different orderings of the resulting merged toolpath. When the toolpaths are merged each of these ordering strategies is calculated and the quickest strategy chosen.

Merging by Part

When the Merge By Part check box is selected, the toolpath merge not only tries to optimize the whole toolpath, it also tries to group related geometry to cut together.

Merge By Part option unchecked: The Squares profiled after all the Circles have been pocketed.
Merge By Part option unchecked: The Squares profiled after all the Circles have been pocketed.
Merge By Part option checked ✓: Each Square is cut after its circles have been pocketed.
Merge By Part option checked ✓: Each Square is cut after its circles have been pocketed.

Merging by part tries its best to respect the ordering of the toolpaths in the toolpath list, and the order of contours within a given toolpath. In particular, if contours of two different toolpaths lie within the same part, the contour of the first toolpath will be cut before the contours of the second toolpath. The following examples show how the toolpath order in the main toolpath list alters the results of toolpath merging.

Merged from main toolpath list going A ► B ► C
Merged from main toolpath list going A ► B ► C
Merged from main toolpath list going B ► C ► A
Merged from main toolpath list going B ► C ► A

Toolpath Name

Enter a name for the newly created merged toolpath.

Feeds and Speeds

It may be that the toolpaths to be merged have different feeds and speeds. Toolpath merging will automatically change the feeds and speeds for the different parts of the toolpath but you should check that your post -processor supports this.

Toolpaths | Moulding Toolpath

This icon opens up the Moulding Toolpath Form. This form is used to create a toolpath from a drive rail and a profile. The result of machining the toolpath is the extrusion of the selected cross-section profile along the pre-selected drive rail. Although strictly speaking the result of this is a 3D shape because it does not use a 3D model it is classified as a 2.5D Toolpath.

Drive Rail Selection

From the 2D view, select the drive rails for the toolpath followed by the profile you wish to extrude. You may select multiple rails. The last selected vector is the Profile that you are extruding.

In the 2D view your rail vector will now be colored orange and will show a green square indicating the start point, along with arrows along the vector showing you the direction.

The direction and start point may not be what you intended, you can change the direction (and start point location on an open vector) by right clicking in the 2D View on the vector and choosing .

The button on the form can be used at any time to empty your current selection; this will deselect the drive rail and if already selected the cross section too. This can be used if you want to change the selection without exiting the form.

Cross Section Selection

After you have chosen your drive rail the next step is to select a cross section that will be swept around the drive rail to create the moulding. The cross section needs to be an open shape in order for this to work.

To select a cross section click on the appropriate vector in 2D View and it will turn orange as with the drive rail, arrows and a green square will appear on it. In addition the drive rail will now have red lines shown on it. These indicate the side of the vector that the shape will be swept along. If this is not correct you will need to reverse the drive rail vector as documented in the previous section.

The arrows and green square on the cross section indicate the direction and the start point. The start point of the cross section will be attached to the start point of the drive rail. If you need to change the start point of the cross section you can do so by selecting the cross section with a right click and choose to Reverse Profile as shown in the image below. Doing this will change the arrow direction and move the green square and also change which end of the cross section is effectively hung on the drive rail when the toolpath is created.

Note

On a closed vector shape, the cross section profile will always hang on the outside of the shape. Therefore, your drive rail vector should always represent the inside edge of the border/frame shape for which you are creating the toolpath. To change the direction in which the toolpath is created, click the Reverse Rail option on a closed vector drive rail.

Toolpath Position

You now need to determine the toolpath position within the material. The Z Height of the toolpath is determined by the height of the selected cross section. You can interactively position the toolpath by pulling on the slider or you can enter exact values in the edit boxes.

Note

If the cross section you have selected is higher than the material thickness then you will need to change your material thickness in the material setup form to accommodate the profile height, or exit the form and edit the height of the cross section vector you are using to create the Moulding Toolpath to fit within the material block.

Selecting a Tool

The next step in this form is to select a tool to finish-cut the moulding shape. This would typically be a ball-nose or tapered ball-nose tool but that may vary depending on the shape you plan to cut. To select a tool use the button to access the Tool Data Base. If the tool you require is already shown as the selected tool, you can use the Edit option to check and/or modify the tool settings for this particular toolpath.

Note

The generated toolpath will follow the shape and direction of drive rail vector. At the end of an open vector it will lift by at least the stepover distance, step over and then come down to the surface again, returning along the vector in the opposite direction, this small lift is designed to avoid leaving connecting marks on the surface of the part and so improve the potential finish quality. On a closed vector after completing a pass the length of the vector it will lift, step-over, return the tool to the profile shape and continue cutting in the same direction - this direction can be reversed by right clicking the drive rail vector and using the Revers Rail option to change the direction of the arrows on the vector.

Close up of calculated toolpath showing lifts at ends of an example created with an open drive rail.
Preview of toolpath created from the cross section and drive rail shown on the previous page.

Vary Stepover

Typically the Stepover value specifies the horizontal distance that the tool will step over and this is projected onto the 3D model. Checking ✓ the Vary Step Over option will instead adjust the step over based on the shape of the cross section profile vector rather than just projecting the standard pattern down Z. In cases where there are steeply curved, angled or near vertical edges this should result in passes that are closer together, in most situations this will improve the finish quality but also potentially increase the machining time

[object Object]
Toolpath calculated with standard Stepover.
[object Object]
The same shape with the Vary Step Over option checked ✓.

Skip Flat Regions

This choice will only become available when the option is checked ✓ to Machine Flat Regions when using the Larger Area Clearance Tool in the next section of the form. When this is active the software will look to identify flat areas of the cross section profile that can be machined with the larger tool. If these regions are detected and Skip Flat Regionsis also checked ✓ then the finish tool will avoid re-machining those flat areas as in most cases they should already have been completely finished by the Larger Area Clearance Toolpath.

[object Object]
Finish toolpath calculated with Skip Flat Regions. This avoids machining these areas if the Larger Area Clearance tool can fit and is selected.

Use Larger Area Clearance Tool

If this option is selected, then two tools are used to cut the shape. In effect the Larger Area Clearance Tool is similar to a 3D Z Level Roughing toolpath and would be cut first. It will use the tool parameters to generate multiple depth 2D pockets following the direction of the selected rail to clear away excess material. This should be used if the material is too deep and/or hard to cut directly with your selected finishing tool. As documented above and below using this option with a flat shaped tool can also be very beneficial to the machining time and finish on cross section profile shapes with flat/horizontal regions.

When you use the option to Use Larger Area Clearance Tool, the software will calculate two toolpaths, the first will have [Clear] in its name to differentiate the two, [Clear] being the toolpath associated with the Use Larger Area Clearance Tooland the other, is the finish toolpath using the smaller tool. The [Clear] toolpath should be run first on the machine:

Machine Flat Regions

If this option is checked ✓ then the software will try to detect flat/horizontal areas in the cross section profile. If the specified Larger Area Clearance Tool can fit into these areas then they will be machined as part of the roughing operation. When using a flat tool this should give both a superior finish and also help to reduce the cutting time. Having this option checked ✓ will also allow you to choose the option Skip Flat Regions in the finish tool section which will stop the secondary toolpath from re-cutting these areas.

Note

This option will override the Machining Allowance value in the flat areas of the shape to ensure they are machined to the correct depth and not left with additional material on.

Ramp Plunge Moves

The Larger Area Clearance Tool can be ramped over the specified distance instead of plunging vertically into the part. For some tool types and shapes, this approach can reduce the heat build-up that may damage the cutter and also reduces the load on the spindle and z axis bearings.

Machining Allowance

The machining allowance is a virtual thickness which is added to the moulding profile when the Use Large Area Clearance Tool is calculated. This ensures that the toolpath leaves some extra material on the part cut with a larger tool.

Note

If you have the option selected to Machine Flat Regions the Machining Allowance will only be applied to the other areas of the cross section profile, on the detected flat regions the software will cut down to the actual surface and ignore the Machining Allowance value within those areas ensuring that they are cut to the thickness specified by the cross section profile vector.

Create Sharp Corners

This option can be checked ✓ when working with rails that have sharp corners, allowing you to force the software to try and emulate these in the Moulding toolpath. Below you can see the effect of checking ✓ this option on a closed vector shape with the standard corners option on the left showing the toolpath rolling around the shape edge and the Sharp Corners option on the left where it has forced mitre style corners in the machined shape.

Moulding Toolpath - Create Sharp Corners Un-Checked
Moulding Toolpath - Create Sharp Corners Un-Checked
Moulding Toolpath - Create Sharp Corners Checked ✓
Moulding Toolpath - Create Sharp Corners Checked ✓

Boundary Offset

This option can be used to force the toolpath to cut past the edge of the part that is parallel to the drive curve vector. By default the center of the tool will go to the edge of the ends of the selected profile vector as its extruded along the drive rail. It may be desirable to extend this distance to either force the tool down the edge of the profile shape with vertical or steep edges or to ensure the toolpath has gone far enough past the edge to cleanly cutout the final shape with a profile toolpath. The value entered for the Boundary Offset will force the tool past the ends by the specified amount. As such if you want to ensure a vertical or very steep edge at your profile ends is machined you will need to specify a value which is at least the radius of your tool plus a small additional amount (say an additional 10% of the radius). For example if you are using a 0.25 inch (6mm) diameter ball-nose tool for the finish cut then you would specify a minimum of 0.15 inch or 3.6mm (= tool radius + 10%) to ensure the tool would be forced down the edges of your shape. If you wanted to ensure the roughing had also been able to machine these areas then the value should be based on your Larger Area Clearance Tool size instead.

[object Object]
With no Boundary Offset the toolpath will not cut down the front and back vertical faces of the shape.
[object Object]
With a Boundary Offset value specified you can see the toolpath cuts over the edges.


Use automatic boundary offset

When this option is selected, Cut2D Pro will calculate the boundary offset to ensure that the tool fully cuts the ends of profile, even if profile ends in vertical/steep edges.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Photo V-Carve Toolpath

The Photo V-Carve toolpath uses the V-bit to etch a copy of the selected bitmap picture into the surface of your material.

Preparing the bitmap

This strategy requires a source bitmap image or photograph to be selected in the 2D View.

Your source bitmap can be edited in a number of ways before using this form to create your Photo V-Carve toolpath. You can use the Crop Bitmap command to trim a bitmap to a vector outline. This will allow you to remove any parts of a bitmap that you do not require.

The Edit Picture tool can also be used prior to creating the toolpath in order to adjust many important aspects of your image - such as brightness and contrast. In addition it can be used to add a feathered border the image. For the best results you should use this tool to highlight and accentuate out the important details of your image before creating your toolpath.

The fields on the form are as follows.

Cutting Depths

Start Depth (D)

This specifies the depth at which the Photo V-Carving toolpath is calculated, allowing Photo V-Carving to be machined inside a pocket region. When cutting directly into the surface of a job the Start Depth will usually be 0.0. If the Photo V-Carving is going to be machined into the bottom of a pocket or stepped region, the depth of the pocket / step must be entered. For example, to carve or engrave into the bottom of a 0.5 inch deep pocket, the Start Depth = 0.5 inches

Max Carving Depth

Max carving depth is the maximum depth the tool will cut into the material. It also impacts the number of lines that can be carved into a job at a specific size.

Stepover Retract

This parameter specifies how much the tool will retract before moving to the next line. This should be set to a value high enough, to allow tool to move safely to start of the adjacent line, but as low as possible to avoid slowing down machining.

Tool

Clicking the button opens the Tool Database from which the required VCarving or Engraving Tool can be selected. See the section on the Tool Database for more information on this.

Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database.

Strategy Settings

Raster

Selecting this option will generate a single set of parallel lines, or stripes, across your selected image.

Hatch

This option will create two sets of parallel lines at 90 degrees from one another. This strategy will generally produce a denser image reproduction, but will typically take twice as long to etch.

Selected Vectors

Selecting this option will generate toolpath along the selected vectors. This is an advanced option that allows to produce special effects, but requires more time to set-up.

Line Spacing

This slider adjusts the gap between the raster stripes - tight striping produces a denser image reproduction, but will take a lot longer to etch. The line spacing is expressed in percentage of the tool width at maximum carving depth .

At 100% the line spacing is calculated to create a 'knife edge' ridge in the deepest regions of the design - no flat left on the material surface. This is the maximum definition / resolution based on the specified Depth.

Increasing the Line Spacing, reduces the number of lines and increase the width of the flat regions on the material surface.

Line Angle

Adjust this slider to change the angle of the stripes or hatching used to etch the image. Zero degrees will produce horizontal stripes and ninety degrees, vertical.

Toolpath Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Pocketing Toolpath

Cutting Depths

Start Depth (D)

This specifies the depth at which the toolpath is calculated from.

When cutting directly into the surface of a job the Start Depth will often be 0. If machining into the bottom of an existing pocket or 3D region, the depth needs be entered.

Cut Depth (C)

The depth of the toolpath relative to the Start Depth.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Pass Depth Control

When a toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description) is used to determine the number of passes needed to profile down to the specified Cut Depth. However, by default the software will also modify the precise step down by up to 15% in either direction, if by doing so it is able to total number of passes required to reach the desired cut depth. It is nearly always desirable to benefit from the significantly reduced machining time of cutting using less passes if possible. Nevertheless, there are some occasions where the exact step down for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section page indicates how many passes will be created with the current settings.Thebutton will open a new dialog that enables the specific number and height of passes to be set directly.

Specify Pass Depths

The Pass Depths section at the top of the form shows a list of the current pass depths. The relative spacing of the passes is indicated in the diagram next to the list. Left click on a depth value in the list, or a depth line on the diagram, to select it. The currently selected pass is highlighted in red on the diagram.

To edit the depth of the selected pass, change the value in the Depth edit box and click .

The button will delete the selected pass.

The Passes button will delete all the passes.

To add a new pass, double left click at the approximate location in the passes diagram that you wish to add the pass. A new pass will be added and automatically selected. Edit the precise Depth value if required and then click .

The Set Last Pass Thickness option will enable an edit box where you can specify the last pass in terms of the remaining thickness of material you wish to cut with the last pass (instead of in terms of its depth). This is often a more intuitive way to specify this value.

Pass Depth List Utilities

This section of the form includes two methods for creating a set of passes in one go.

The first method simply sets the passes according to the Pass Depth property of the selected tool. By default, this is the method used by Aspire when it creates profile passes initially. However, the Maintain exact tool pass depth option checked, ✓ the software will not vary the step size to try and optimize the number of passes (see above).

The second method creates evenly spaced passes according to the value entered in the Number Of Passes edit box.

To apply either method click the associated button to create the resulting set of pass depths in the passes list and diagram.

Note

Setting the number of passes with either of these utilities will discard any custom passes you may have added.

Use Larger Area Clearance Tool

If this option is selected two tools are used to clear the pocket. A large tool to do the bulk of the area clearance and a smaller tool (the first tool selected) to remove the remaining material and do a final profile pass.

When a pocket toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description in the Tool Database) is used to determine the number of passes needed to pocket down to the specified Cut Depth. However, by default Cut2D Pro will also modify the tool step down by up to 15%, if by doing so it is able to reduce the total number of passes required to reach the desired cut depth. It is usually desirable to benefit from the significantly reduced machining time of cutting pockets using less passes if possible.

Nevertheless, there are some occasions where the exact step downs for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section of the Pocket Toolpath page indicates how many passes will be created with the current settings. The button will open a new dialog that enables the specific number and height of passes to be set directly.

Clear Pocket

There are two choices of the type of fill pattern that will be used to clear away the area to be machined with the Pocket Toolpath, Offset and Raster.

Clear Pocket - Offset Strategy
Clear Pocket - Offset Strategy
Clear Pocket - Raster Strategy
Clear Pocket - Raster Strategy

Offset

Calculates an offset area clearance fill pattern to machine inside the selected vector(s). Options for Cut Direction to be either: Climb (CCW) cutting direction Conventional (CW) cutting direction.

Note

When the stepover for a pocket fill is greater than 50% of the cutter/tip diameter the software automatically adds 'Tail' moves to the corner regions on the toolpaths to ensure material is not left on the job. You can see these in the diagram of a star being pocket machined below:

Offset larger than 50%
Offset larger than 50%
Tails to clean out corners
Tails to clean out corners

Raster

Calculates a Raster based area clearance fill pattern to machine inside the selected vector(s). Cut Direction for the final pass to be either:

  • Climb (CCW) cutting direction
  • Conventional (CW) cutting direction

Raster Angle

Between 0 and 90°, where 0° is parallel to the X axis and 90° parallel to the Y axis.

Profile Pass

This option is used to leave material on the inside of the pocket for the Profile Pass to clean-up. This is often very useful for ensuring the cutter does not mark the edge surface of the pocket when roughing out.

Pocket Allowance

This option is used to leave material on the inside of the pocket for the Profile Pass to clean-up. This is often very useful for ensuring the cutter does not mark the edge surface of the pocket when roughing out.

Ramp Plunge Moves

The cutter can be ramped over a distance into the pocket instead of plunging vertically. This approach reduces heat build-up that damages the cutter and also reduces the load on the spindle and z axis bearings.

Use Vector Selection Order

If this option is checked, ✓ pockets will be machined in the order you selected them. If the option is not checked the program will optimize the order to reduce machining time.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Preview Toolpaths

Calculated toolpaths can be previewed to see exactly what they will produce when cut into the material. The 3D preview mode also allows the job to be viewed in different material types with the option to paint the machined regions with a Fill Color

Material Selection

The pull-down list offers a range of material types to shade the 3D model.

[object Object]

Use Solid Color

If this is selected the color for the material can be selected from the color picker below the list.

Use material

The user can choose from the list of pre-defined material effects by clicking on appropriate position on the list. These include many wood grains, metal effects, stone and plastic.

Adding Custom Materials

Additional materials can be added to the library using the list itself. You can add a category (folder) which groups your textures using <Create mew category...>. You can also add extra textures under any category using <Add new texture...>.

Alternatively, you can copy an image file (JPG, BMP or TIF) of the material or image you wish to render the job with into the Textures folder within the 'Application Data Folder'. You can open the Application Data Folder from within the program using the File ► Open Application Data Folder menu command.

Shading textures can be obtained from sources such as the internet, clipart libraries or simply create your own from a digital or scanned photographs. For good quality results the image needs to be approximately 1000 pixels x 1000 pixels. The texture image is simply scaled proportionally in X and Y to fit the longest side of the job.

Machined Area Color

Material Color

With this setting, the areas of your preview will simply be colored using the material defined above. Effectively this switches off independent material settings for your machined areas.

Global Fill Color

Paints all the machined regions with the selected color. Selecting the associated pull-down list opens the default color selection form. Click on one of the preset colors, or click to create a completely custom color.

Toolpath Color

If this option is selected, each toolpath can have a different color assigned. If the 'No Fill' option is selected from the color picker form, the current toolpath will be shown in the material color.

Choose the color you want for the fill of that toolpath and it will be applied to the areas that the toolpath has carved when they are previewed. Once you assign an individual color a small square of that color will be displayed next to the name in the toolpath list. This can be seen top left of each tool icon:

Animation Settings

Animate preview

This option will show the material being removed by the cutter as the preview is drawn.

Draw tool

This option will show a wireframe animation of the tool (to scale) cutting the job.

Toolpath Preview Tools

Preview Toolpath

This option animates the selected toolpath cutting into the material

Preview Control Simulation

The preview controls provide full video-like playback control of your toolpath. You can use this mode to analyze the tool moves in detail, step-by-step. To begin using Preview Control, click on either the Run, Single Step or Run to Retract buttons

Begins Preview Control simulation
Begins Preview Control simulation
Moves the toolpath on by one tool move.
Moves the toolpath on by one tool move.
Runs the toolpath to the next retract move, then pauses the tool.
Runs the toolpath to the next retract move, then pauses the tool.
Temporarily halts the tool in its current position and enables the Stop button so you can exit Preview Control mode
Temporarily halts the tool in its current position and enables the Stop button so you can exit Preview Control mode
Exits Preview Control mode.
Exits Preview Control mode.

Preview All Sides

This option animates all calculated toolpaths cutting into the material on both sides if working in a two sided environment without being in the 'Multi Sided View' mode (This option will be grayed out if working in a single sided setup)

Preview All Toolpaths


This option animates all calculated toolpaths cutting into the material


Preview Visible Toolpaths

Previews all the visible toolpaths

Reset Preview

Resets the material back to a solid block

Save Preview Image

Saves an image of the 3D window as a BMP, PNG, JPG or GIF file

Toolpaths | Prism Carving Toolpath

Prism carving gives a raised 'bevel' effect to shapes and letters similar to a 'hand carved' look.

Prism Carving uses an angled tool to create a raised prism shape on the top of the selected vectors. The tool will profile at a given depth creating a nice sharp finished shape such as the lettering shown in the image below. This is often paired with a Profile or Pocket toolpath to carve the vertical edge around the shapes or clear out the material between them. This type of toolpath is often, though not exclusively, used on lettering.

Cutting Depths

Start Depth (D)

Start Depth (D) specifies the depth at which the Prism Carving toolpath is calculated from. When cutting directly into the surface of a job the Start Depth will often be Z0. If machining into the bottom of an existing pocket or stepped region, the depth of the pocket/step that you are starting from must be entered here.

Prism Depth

This sets the depth of the Prism Carving toolpath relative to the Start Depth, the total depth of the base of the prism shape (within the material) will be the combination of the Start and Flute Depth. This depth is particularly important to set correctly as if it is too shallow then the prism shape may be truncated so it will have a flat top (shown in the image below right). The minimum depth needed to avoid this is determined by the widest point on the vector/s selected (W) and the angle of the tool (A). This can be calculated automatically by using the Set Depth for Full Prism function (see below for more details).

Full Prism
Full Prism
Truncated Prism
Truncated Prism

Set Depth for Full Prism

For this button to work you both need to select the vectors you plan to toolpath and also have selected the tool you are going to use, then when you click it, the Prism Depth will be set to the minimum required to ensure a full point on the prism for the current selection/tool.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Cut Direction

The direction of cut can be set to either Conventional or Climb machining, the choice for this will largely be dictated by the material being machined and the type of tool being used. See the section on Profile Toolpaths in the Reference Manual for more information on the differences between these.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Quick Engraving Toolpath

This form is used specifically for calculating engraving and marking toolpaths.

Depth / Pressure

When using Conventional Engraving and End Mill cutters the Depth to engrave / mark is specified and this z depth dimension is output in the toolpath file sent to the CNC machine. The 3D Preview of these toolpaths shows the specified depth of engraving.

When using a Diamond Drag marking Tool the Pressure setting is used to pre-load the spring to ensure the tip of the diamond stays in contact with the material surface, especially when marking uneven surfaces. The 3D Preview of the depth these toolpaths will mark using the Angle of the diamond and the Width of the Line.

For example, when using a 90° Diamond Drag Tool with a 0.010 inch Line Width specified. The depth shown in the 3D preview will be 0.005 inch (with 90° the depth = half the line width).

The ratio of Depth to Line Width will change when using diamond drag tools with different tip angles. When the option to use a Nose Cone is selected (see below) the actual depth specified on the form is used when previewing the toolpath in the 3D view.

Strategy

When using the Quick Engraving Form the Stepover for the cutter is specified on the form and is NOT automatically set from the Tool Database.

The selected text or vectors can be Outlined or Filled.

Outline

The tip of the cutter runs on the selected lines engraving / marking the material surface

[object Object]
Example of outline engraving

Fill

A pattern is used to engrave / mark inside the selected text or vectors. There are 3 fill pattern options.

[object Object]
Fill engraving with Offset pattern
[object Object]
Fill engraving with 45° Hatch pattern
Fill engraving with Cross Hatch pattern. Cross Hatch Fill pattern engraves 2 sets of lines, with the second set at 90° to the angle specified.

Use Nose Cone

A nose cone is often used when engraving or marking material that is not flat. The nose cone is spring loaded forcing it to slide on the surface of the material. The engraving cutter is set to extend / protrude out of the bottom of the nose cone by the depth of engraving / marking required. This is typically set at around 0.010 inches to 0.020 inches.

When the option to use a Nose Cone is selected the actual depth specified on this region of form is used when previewing the toolpath in the 3D view.

Number of Passes

This option runs the cutter multiple times divides over the toolpath pattern.

Immediate Output

Once calculated, your toolpath is stored in the central Toolpath Tree and can be saved, edited or output to your machine at anytime using the command. In addition though, this form also includes a convenient Immediate Output section that allows you to save or send the most recently calculated toolpath directly from this form without having to close it.

Post Processor

Use this drop-down list to select the post-processor for your machine.

Add side to toolpath name

If you are creating aligned toolpaths for a two-sided part, this option automatically adds the side name to the toolpath name as it is saved or exported to help keep your toolpaths organised.

Output direct to machine

If your post-processor supports direct access to your cnc machine (including machines supported by VTransfer), this option will be available. Selecting this option will bypass saving the toolpath to disk and instead send it straight to the direct output driver.

Toolpaths | Recalculate All Toolpaths

This command forces a recalculation of all the toolpaths in the Toolpath list. It is useful when the artwork used by the toolpaths has been modified, or the material block settings have changed.

Toolpaths | Save All Visible Toolpaths as a Template

The Toolpaths ► Templates ► Save All Visible Toolpaths as Template menu command (or the associated icon) allows a group of toolpaths to be saved as a single template. As an example, the toolpaths may have all the settings used for Profiling and Pocketing operations for a particular type of job and material combination. These toolpaths settings can then be recalled simply by opening the template and selecting the appropriate vectors for each toolpath.

If toolpaths with the Vector Selection mode set to Automatic are saved as templates, these setting are saved with the template. When the template is re-opened and the toolpaths recalculated, they will automatically select all vectors which match the filters specified with the Vector Selector for that toolpath.

Multiple Sheets

If there are multiple sheets a message will be appear asking if you want to apply the template to every sheet in the job. If 'yes' is chosen the template will be applied to all the sheets and any toolpaths will be automatically calculated where possible. The toolpaths generated for each sheet will be prefixed by "Sn-" where 'n' is the number of the sheet for the toolpath. E.g if the template has a toolpath called "Cut Out" the associated toolpaths for each sheet will be:

"S1-Cut Out", "S2-Cut Out" etc.

If the template contains toolpaths that reference layers which do not exist in the current file the missing layers dialog will appear once and the option chosen will be used for every sheet the template is applied to. Choosing either 'Create the missing layers' or 'Load the toolpaths without creating missing layers' will mean that any toolpaths which reference those layers will be created as empty and have the visibility set to off.

If the toolpaths in the template use automatic vector selection then vectors matching the selection criteria can be created and the empty toolpath recalculated. If not using automatic selection an empty toolpath can be edited by double clicking on its name in the toolpath list or selecting the Edit Toolpath icon in the Toolpaths tab. Once the toolpath form is open, the vectors to be machined can be selected and the toolpath calculated using all the saved settings.

Toolpaths | Save Toolpath Template

Using the Toolpaths ► Templates ► Save Selected Toolpath as Template menu command (or the associated icon), all the settings for the currently selected toolpath can be saved as a template.

Toolpaths | Save Toolpaths


This option allows toolpaths to be saved in the appropriate file format needed to drive the CNC machine. Toolpaths can be saved as individual files for each tool used or as a single file containing multiple toolpaths for CNC machines that have automatic tool changers.

Individual Toolpaths

CNC machines that require the tooling to be changed manually will typically need a separate toolpath for each cutter used. The procedure for saving this type of toolpath is to:

  • Select the toolpath to save from the Toolpath List
  • Click on the Save option and the Save Toolpaths form is displayed.
  • Select the correct Postprocessor for the CNC machine from the pull-down list
  • Click the Save Toolpath(s) button
  • Enter a suitable Name and click the button

Note

When multiple toolpaths are created using the same tool geometry and tool number, they can be saved into a single file by selecting the option to - Output all visible toolpaths to one file.

Automatic Tool Changing Support

CNC Machines that have Automatic Tool Changing (ATC) capabilities can work with a single file that contains multiple toolpaths, each having a different tool number.

The postprocessor must be configured to support ATC commands for your CNC machine. Contact your software or machine supplier for more details.

  • The procedure for saving these toolpaths is,
  • Use the Up and Down arrows to order the toolpath list in the cutting sequence required.
  • Tick each toolpath to ensure it is drawn / visible in the 3D window as shown:
  • Click on the Save option and the Save Toolpaths form is displayed. Select the option Output all visible toolpaths to one file

The names of the toolpaths that will be written into the file are displayed along with the tool number in square brackets [1]. If a calculated toolpath is not required, simply tick to undraw it.

Click the button Enter a suitable Name and click the button

Error Messages

The postprocessor automatically checks to ensure:

  • It has been configured for saving files that include ATC commands
  • A different tool number has been defined for each different cutter being used.

An error message will be displayed to indicate the problem if either of these items is not correct.

Toolpaths | Texture Toolpath

The 3D Texture Machining functionality uses a specialized toolpath algorithm and the shape of the tool to generate a textured finish on the part.

Tool

Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.

Texture Settings

Use selected vectors as pattern

By default this option is unchecked and the texture form will generate a random texture pattern using any selected vectors as a clipping area. If this option is checked, ✓ the currently selected vectors will be used as the pattern for the texture and the only options available will be 'max. Cut Depth' and 'min. Depth' to control the depth of the cuts along the selected vectors.

Ramp at start and end

This option is only available when using selected vectors as patterns. If this option is checked ✓ each of the selected contours is cut using a fluting move, otherwise each of the contours is cut with a regular profile move. The resulting textures may look very different because of this small change.

Ramp at start and end switched on
Ramp at start and end switched on
Ramp at start and end switched off
Ramp at start and end switched off
Ramp at start and end switched on
Ramp at start and end switched on
Ramp at start and end switched off
Ramp at start and end switched off

Max. Cut Depth

The maximum depth any of the carved scallops will be machined to and is specified in the job units.

Min. Depth

Using the slider this is specified as a percentage (%) of the Max. Cut Depth and controls the minimum depth any of the scallops will be machined to.

Note

For example, with a Max Cut Depth = 0.200 inches and a Min Cut Depth of 0.050 inches, the depth of the carved scallops will range randomly between 0.200 inches and 0.050 inches.

Max. Cut Length

Specifies the maximum length for any of the carved grooves and is specified in the job units.

[object Object]
Max. Cut Length between the lines

Min Length

Using the Slider this is specified as a percentage of the Max Cut Length and controls the minimum length any of the carved grooves.

Max. Overlap %

The percentage (%) of the Max Cut Length that each scallop is allowed to overlap the adjacent scallop running along the cutting direction. Where, 1% will result in almost zero overlap of adjacent scallops 50% will result in some of the scallops being machined half way over the adjacent scallop.

Variation

Using the slider this is specified as a percentage of the Max Overlap. Overlap variation of 100% = the Max Overlap and random pattern Overlap variation of 1% = No Overlap and an almost constant pattern.

Stepover

The distance between each parallel set of lines of carved scallops.

Angle

The direction the texture is machined across the surface, an angle of zero is parallel to the X axis, examples of setting the angle to 45 and 90° can be seen below.

Boundary Vector Offset

If you enter a value in this field, the texturing will be offset from the boundary by the specified amount. If you are texturing in a recess, you should enter a value here up to the radius of the tool to avoid the walls of the recess being damaged by the tool.

Position and Selection Properties

Safe Z

The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.

Home Position

Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.

Vector Selection

This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.

Name

The name of the toolpath can be entered or the default name can be used.

Toolpaths | Tool Database

The Tool Database is used to make cutter management and selection very quick and easy, and reduces the possibility of programming jobs with incorrect cut depths and speeds and feeds. It allows pre-defined tools and settings (speeds, feeds, stepover etc.) to be selected from a list for a given machine / material.

The Tool Database can be accessed from the button through the various Toolpath forms. You can open the Toolpaths Tab button or through the Toolpaths menu.

Overview

This is a summary of the main entities and relationships in the database. More details on those will be given in the next sections.

  1. Tool geometry entities (organised hierarchically in the tree).
  2. List of Materials (Managed through the Material Management dialog).
  3. List of Machines (Managed through the Machine Management dialog).
  4. Cutting Data set for each tool geometry. This includes the Cutting Parameters, and Feeds & Speeds, and are defined per machine / material.

Tool Properties are divided into two categories,

  1. Tool geometry: This is the physical properties of the tool such as the diameter, tip radius, etc...
  2. Cutting data: These include the Cutting Parameters and Feeds & Speeds of the tool. These values are defined for a particular material / machine.

Apply Changes

If you modify the Tool database, your changes will only be saved if you click OK. If you exit the Tool Database window using the Cancel button, any changes you have made since opening the Database will be discarded.

Tool Tree

The Tool Tree is located on the left-hand side of the Tool Database. Click on items in the list to see or edit their properties using the Tool Info section of the database window.

You can drag items up and down the list to change their order or drag them inside / outside of groups.

New Tool

Create a new tool with the default name for its type. The tool will be created with the first available type by default, but that can be changed through the Tool Type dropdown to the desired type.

Copy Tool

Duplicate the selected tool geometry or group in the list. If you're copying a tool, it will be copied without its cutting parameters.

The cutting parameters can be subsequently be,

  • Copied from the same tool, different material.
  • Tool with identical geometry, any material.
  • Created with default values.

Delete Tool

Delete the tool as well as all of the cutting data for all machines / materials for which it was defined. If we're deleting a group, this will delete all the tools inside it in the same way.

New Tool Group

Create a new group in the tool database. Tools can then be dragged inside the newly created group. Alternatively, select the group and create a new tool directly under the selected group.

Export Tools

Export an individual tool or an entire group to a tool database file.

Import Tools

A tool database file can be imported into the currently open tool database. You will have 3 options,

  1. Import: This will simply import the given tools under the selected group (or as a top-level tool / group).
  2. Merge: This will attempt to merge the incoming tool group hierarchy with the current one (without any regards for selection)
    1. Overwrite: When it's faced with two similarly nested tools that have the same tool geometry, the cutting data of the incoming tool will overwrite the current tool's cutting data for the active machine / material.
    2. Without overwriting: A new machine / material will be created to contain the cutting data of the incoming tools.

Tool Definition

When a tool or group is selected in the Tool List, its properties are displayed in the Tool Info section on the right-hand side of the Tool Database.

Name

This will go to the Name Format dialog to edit the name template for this tool type.

The name displayed here is then a result of evaluating the template in the current context (active machine, material and the cutting data defined for those as well as the tool geometry).

The name of a tool group can be defined directly through this dialog.

Tool Type

Various cutters can be specified in the database. Changing the cutter tool type is equivalent to creating a new tool, so all existing data for that tool (if any) may not be applicable anymore.

V-Bit
V-Bit
Engraving
Engraving
Tapered Ball Nose
Tapered Ball Nose
Ball Nose
Ball Nose
End Mill
End Mill
Radiused End Mill
Radiused End Mill
Form Cutters
Form Cutters
Diamond Drag
Diamond Drag
Drills
Drills

Notes

The tool notes section simply allows you to save any additional text descriptions, special instructions or relevant information you may require, within your tool definition.

Diameter

The diameter of the tool in either inches or mm. The tool image will indicate where this dimension is taken from.

Number of Flutes

The number of Flutes for the bit. This is particularly useful if you would like to calculate a Chip Load value.

Cutting Data

The cutting data is the set of parameters which can differ between materials and machines. This set of parameters are defined to be per machine per material. The visible set of parameters are the ones for the active material / machine.

Creation / Copying

The cutting data is defined per material per machine. If the data is not defined already for a tool, we create it in a number of ways,

  1. Create with some default values which you can then change for your purposes.
  2. Copy from the same tool from a different material: This could be a sensible starting point if the materials have similar / close hardness.
  3. Copy from a different (identical) tool from the same (or different material)

Pass Depth

The maximum depth of cut the tool can cut. The Pass Depth controls the number of z level passes that are calculated for a toolpath.

For example, creating a pocket 1 inch (25.4 mm) deep using a tool that has a Pass Depth of 0.25 inches (6.35 mm) will result in the toolpath making 4 passes.

This value can be defined per machine / material depending on the machine's rigidity and the material's hardness.

Stepover

The distance the cutter moves over when doing area clearance cutting. For example, when raster machining the cutter will machine along the X axis, stepover in the Y direction and return parallel to the first line of cut. The greater the stepover the faster the job will be machined, but this must be balanced with the material being cut and the tooling being used, to ensure that the tool does not break. Therefore, this property (along with all other Cutting Parameters can be defined per material / machine).

When stepover's greater than 50% of the cutter / tip diameter are used the software automatically adds 'Tail' moves in the corner regions of toolpaths to ensure material is not left on the job for offset based strategies.

When using V-Bit Tools, the Stepover fields automatically change to use the following options.

Final Pass Stepover

The distance the cutter moves over when finish machining and is usually set to be a relatively small distance to produce a smooth surface finish on the job.

Clearance Pass Stepover

Only used when a V-Bit tool is being used to rough machine at multiple Z levels down to a specified flat depth. This stepover can be much larger than the Final Pass Stepover because the tool is only rough machining material away. Increasing the Clearance Pass Stepover will reduce the machining time, but you must be careful to ensure it is not too great for the material being cut.

Spindle Speed

Speed of tool rotation, specified in revolutions per minute.

Feed Rate

The surface cutting rate at which the cutter is moved in the material. The units can be specified in distance per second or minute.

Plunge Rate

The cutting rate at which the cutter is moved vertically into the material or during ramping moves. The units can be specified in distance per second or per minute.

Material / Machine

The Feed rate and Plunge rate you should use will vary depending upon the material being machined and the tooling being used.

Chip Load

This is the calculated Chip Load based on the entered values for the Number of Flutes, Spindle Speed and Feed Rate. This is displayed to conveniently be able to compare it with manufacturer-recommended Chip Load Values.

Maximum Burn Rate

This is the maximum speed at which the tool, when at 100% power, will still burn the material. This value is used for simulation purposes only. It should be calibrated to match your laser and material. A larger value will result in the simulated toolpath appearing darker.

You will need access to the Laser Module to create and simulate laser toolpaths.

Tool Number

This is the number of the tool needed to machine the job. When using a CNC machine with an Automatic Tool Changer (ATC), it is critical that the correct tool required to cut the job is located in the corresponding carousel location.

Per Machine

This parameter only needs to be defined per machine and so is shared between materials (unlike other cutting data parameters which are defined per machine per material).

Material / Machine Management

The cutting parameters / feeds & speeds section of the tool properties is defined for the active machine / material. This allows you to setup your tools with different values for each material or machine and switch between easily depending on the material you're going to use for the current job.

Material

The combo box is used to change active material. This can also be done by going to the Material Management dialog where materials can be added, removed or edited.

Machine

The combo box is used to change active machine. This can also be done by going to the Machine Management dialog where machines can be added, removed or edited.

Online Tool Database

The tool database can be stored and linked to your portal account so that it can be retrieved at any point from a different installation. For this, the software needs to be logged in to the portal account. Then, the database can be uploaded / download on request.

Login

Login to the portal to be able to access the currently stored tool database and / or upload your existing local one.

Download

Download the tool database stored on your portal account to replace your existing local tool database. This can be used for when we know there is a more up-to-date version online.

Upload

When changes have been made to the tool database, this will upload it to the portal account so that it can be downloaded from any other location linked to the same portal account.

Using Form Cutters

Form Cutters can be added to the Tool Database so that industry standard Ogee and Round-over type cutters, plus user definable custom shapes can be used for edge profiling and decorative carving.

Examples of these types of cutters and the kind of cuts they can be used for are shown in the images below:

Round-over
Round-over
Ogee
Ogee
Profile Cutting Strategy with Form cutter
Profile Cutting Strategy with Form cutter

Custom Form Cutters

Before opening the tool database, draw to exact scale the Right side of the cutter geometry in the 2D Window Use the Node Editing tools to create the arcs and curves etc.

Geometry

Only draw the Right-hand side of the cutter geometry to the correct size and scale as shown in the image above. The shape can be a combination of Lines, Arcs and Bezier spans.

Select the vector, then open the Tool Database dialog and create a new tool. Then, set its type to Form Tool.

The selected geometry will be imported and a profile displayed in the window. Give the Cutter a meaningful name. Enter the cutting parameters - speeds and feeds etc for the various materials you've got defined.

Click the Apply / OK button to save the new cutter into the database list so it can be used at any time.

Toolpaths | Tool Database - Machine Management

This dialog is used to edit and manage the list of machines for use in the tool database. It can be accessed through the Toolpaths Menu or the Tool Database dialog.

Machine List

List the machines added to the database. Selecting a machine activates it. This allows it to be edited in this dialog. In the Tool Database dialog, it results in switching the cutting data of the tools to be the set defined for the active material / machine (if any).

Add Machine

Add a new machine to the database and makes it active ready for editing.

Duplicate Machine

Duplicates the active machine and makes the new machine active ready for editing.

Copy Cutting Data

This could optionally duplicate all the cutting data associated with the original machine for all the tools so that there is a new set of cutting data for the new machine as well.

Delete Machine

Delete the active machine and activate the next one up in the list.

Deleting Cutting Data

This is a destructive process deleting all the cutting data associated with this machine across all the tools.

Name

Allows us to set the active machine's name (if any). Two machines cannot have the same name.

The remaining parameters are optional and can be left empty. They define various common properties of the machine which may help you to identify them and us to tailor the behaviour in future versions.

Apply Changes

Apply changes by clicking or . Clicking will discard any changes made.

Toolpaths | Tool Database - Material Management

This dialog is used to edit and manage the list of materials for use in the tool database. It can be accessed through the Toolpaths Menu or the Tool Database dialog.

Material List

List the materials added to the database. Selecting a material activates it. This allows it to be edited in this dialog. In the Tool Database dialog, it results in switching the cutting data of the tools to be the set defined for the active material / machine (if any).

Add Material

Add a new material to the database and makes it active ready for editing.

Duplicate Material

Duplicates the active material and makes the new material active ready for editing.

Copy Cutting Data

This could optionally duplicate all the cutting data associated with the original material for all the tools so that there is a new set of cutting data for the new material as well.

Delete Material

Delete the active material and activate the next one up in the list.

Deleting Cutting Data

This is a destructive process deleting all the cutting data associated with this material across all the tools.

Name

Allows us to set the active material's name (if any). Two materials cannot have the same name.

Apply Changes

Apply changes by clicking or . Clicking will discard any changes made.

Toolpaths | Tool Database - Name Format

This dialog allows the editing of the name template used for naming tools with that tool type. It can be accessed through the name icon on any of the tools on the Tool Database dialog, and it will affect that particular tool or all tools with the same type.

Format

This field allows entering the name format / template that will be used for this tool (or tools of this type, controlled by the checkboxes).

The template contains variables of the format {Variable Name} which will be substituted by their real value for the tool.

  • For example, {Tool Type} will be End Mill for an End Mill tool and Ball Nose for a Ball Nose tool.
  • We can optionally format those the values in certain ways using modifiers {Variable Name|Modifier}. In the above example, {Tool Type|U} would result in END MILL or BALL NOSE.

The list of all available variables and modifiers is available at the bottom of the page. It can also be accessed by right-clicking the field and selecting the variable.

Variables could relate to the tool geometry, cutting data or even machine and material being used. The tool name will automatically update within the current context. For example,

  • We have materials MDF and Oak and a tool with the name template {Tool Type} {Diameter} {Material Name}. The tool is an 0.5 inch End Mill.
  • When the MDF material is active, the name of the tool becomes End Mill 0.5 MDF. When it Oak is active, it becomes End Mill 0.5 Oak.
  • When the tool is selected for toolpathing, the name of the tool with the correct material name will be used allowing you to see straight away which variant of the tool you've used.

Set as Default

This dialog can be used to manage name formating for each tool type. When a format is set as the default, any subsequently created tools will be named according to that format by default. Setting a format as a default (optionally) allows you to do just that.

Any tool which does not have the default name format for its type can be restored using the next to the format field.

Update existing tools

When changing the name format of a tool, there is the option to rename all the other tools with with the same Tool Type.

If you select this, you will have the option to either

  1. Rename all the tools that had a matching name.
  2. Rename all the tools indiscriminantly.

List of Variables

This is the full list of variables that can be used in the format.

In some cases, we may not be able to find a valid value. For example, if we use the {Material Name} when no material is active. In that case, we will simply keep the variable name in the tool name. This should not happen if the tool is valid / suitable for toolpath selection.

Variable

Type

Geometry

{Tool Type}

String

{Units}

String

{Units Short}

String

{Diameter}

Float

{Included Angle}

Float

{Side Angle}

Float

{Tip Radius}

Float

{Flat Diameter}

Float

{Num Flutes}

Integer

{Max Power}

Integer

Cutting Parameters

{Length Units}

String

{Length Units Short}

String

{Pass Depth}

Float

{Stepover}

Float

{Final Pass Stepover}

Float

{Clearance Pass Stepover}

Float

{Num Passes}

Integer

{Kerf}

Float

{Line Width}

Float

Feeds & Speeds

{Rate Units}

String

{Move Speed}

Float

{Plunge Rate}

Float

{Spindle Speed}

Integer

{Spindle Direction}

String

{Power}

Float

{Maximum Burn Rate}

Float

{Tool Number}

Integer

Material

{Material Name}

String

Machine

{Machine Name}

String

{Machine Model}

String

{Machine Make}

String

{Machine Controller}

String

List of Modifiers

Modifiers can be used on any variable. Valid modifiers depend on the type of the variable.

Variable Type

Modifiers

String

U Uppercase

Example: {Tool Type|U} => END MILL

L Lowercase

Example: {Tool Type|L} => end mill

Float

00.00 Padding / Decimal Points

  • The number of zeros to the left of the dot control the padding.
  • The number of zeros to the right of the dot control the number of decimal points.

Example (For a 1.5101 diameter),

  • {Diameter|0.00} => 1.51
  • {Diameter|0.0} => 1.5
  • {Diameter|00.0} => 01.5

F Fraction in inches

Example (for an 1/8 inch diameter):

  • {Diameter} => 0.125
  • {Diameter|F} => 1/8

Toolpaths | Toolpath List

The Toolpath List is located at the bottom of the Toolpath Tab below the Operations section (toggle tab visibility using Shortcut key F12).

This area displays in a list, the name of each calculated toolpath with a check-box to turn the visibility of the toolpath in the 3D View on and off. The icon next to the check-box shows the type of tool selected for that particular toolpath.

Double-Clicking the name of any of the toolpaths will open up the toolpath strategy window for that toolpath and allow edits to be made to it.

Right-Clicking on the toolpath shows a menu which is described in more detail in the Right Click Menus Page.

Up and Down Arrows

The up and down arrow buttons to the right of the window allow the user to move the selected toolpath up and down in the list.

This will affect the order the Toolpaths are previewed in and if multiple toolpaths are saved as a single file, then this will be the order that the machine cuts them in.

Resizing

You can adjust the space available for the Toolpath list by clicking and dragging the divider that separates the Toolpath List from the Toolpath Operations section, up or down.

Two-Sided Job

The toolpath list shows the list of toolpaths on the current side only. The label at the top will change to indicate whether you're viewing the Top / Bottom sides. To view the toolpaths on the opposite side, just switch sides from the View Toolbar.

Toolpaths | Toolpath Templates

Toolpath templates allow you to improve the efficiency of your production processes by saving the complete toolpath settings for common operations. These settings can then be re-used at any time on different design geometry. Frequently used strategies and tooling can thus be applied to similar jobs, quickly and easily.

The operations you can do with templates include Loading toolpaths from templates, Saving a toolpath to a template and Saving all visible toolpaths to a template.

Toolpaths | Toolpath Tiling Manager

Using the Toolpath Tiling options it is possible to machine objects and designs that are many times larger than the available area of your CNC machine bed. This process is also invaluable if the maximum size of your material pieces are limited. In both cases, a much larger project can still be achieved by breaking the toolpath down into manageable tiles or strips, each of which can fit within the machinable area of your CNC machine, or on the available material blocks. Once cut, the tiles can then be re-assembled to form the finished piece.

The process of tiling begins by creating toolpaths based on the final object entirely as normal - at this stage you do not need to take any account of the available machining bed size. Once you have calculated required toolpaths, click on the toolpath tiling button in the toolpaths pane to open up the toolpath tiling form.

Tiling Options

There are three layout strategies for tiled toolpaths, the most appropriate one will depend on your machines capabilities and the available material.

Individual Tiles

The first tiling option is for individual tiles. This splits the current job in both X and Y, to form a series of entirely separate toolpaths. This is generally the preferred option if you have independent pieces of material to machine, or if you have a moving-bed type CNC machine that will not allow you to 'overhang' material outside of the machinable area.

With this option selected, you are asked to specify the width and height of each tile, and the required overlap (which will be applied in each direction). Tiles are created from the bottom left of your model. The overlap for independent tiles is particularly important for 2.5D toolpaths that utilize the shape of your tool bit (such as V-bit carving). 2.5D toolpaths will need to 'overrun' the edges of your tile in order to complete their cuts using the side of the bit. For this reason, the overlap distance for Independent Tiles will typically need to be at least equal to the radius of your tool bit.

Feed-through in X or Feed-through in Y

Instead of cutting a series of individual pieces of material and assembling them later, it can also be convenient to cut a single strip of material using a series of set-ups - moving the material through the machinable area between cuts. Aspirespecifically supports this technique using the Feed-through in X/Y options. In these cases you will only need to define either the Tile Width or Height (which corresponds to your intended feed-through distance), as the other dimension is assumed to correspond to the shorter side length of your material and will match the equivalent current job dimension. Similarly, the overlap distance is only applied in the direction of the draw-through. Because you will typically be cutting the same piece of material with each toolpath tile, the overlap distance for Feed-through is not as critical as for Individual tiles and is typically used to allow for a margin of error in your set-up accuracy.

Once you have set your tiling option, click the Update Tiles button to see your settings reflected in the Tile Previews in either the 2D or 3D Views.

Tile Previews

The 2D View indicates how the model area is split into tiles. The yellow lines indicate the tile sizes, but the light red areas also indicate the overlap region for each tile.

Double-clicking on a tile will make that tile the active tile.

In the 3D view the toolpaths will be showed tiled, with only the moves that are within the active tile shown.

Simulating Tiled toolpaths

You can also view and simulate individual toolpath tiles in the 3D View. To view the toolpath tiles, simply ensure that the toolpaths are visible (checked ✓ in the Toolpath List) and then select the tile you wish to see either from the Tile Toolpaths form, or the 2D View (see above).

Since tiles are created so that they will all be cut within the same machinable area (i.e. they are all located in a similar position relative to the machining origin), this can make them difficult to visualize using Preview Toolpaths. Simulating each toolpath tile in its absolute position will result in the toolpaths being cut in the same region of your preview block and they will overcut the same area. The Tile Toolpaths form has an option Draw toolpaths in original position for visualization to allow you to simulate the tiles as if they were arranged in their final pattern. With this option enabled, you can visualize how your final piece will look by previewing all your toolpath tiles together, but you should note that it will not reflect the true offset of each toolpath from your machining orig

Saving toolpath tiles

Provided you have created toolpath tiles using the Tile Toolpaths form, an additional option, Output Tiled Toolpaths, will be available in the toolpath saving form.

It will be checked ✓ or unchecked to match the current state of the Tile Toolpaths check box in the Tile Toolpaths form.

Toolpaths | V-Carve Toolpath

This icon opens the V-Carving Toolpath form which is used to specify the type of carving required, , cutting parameters and name for the toolpath.

tgsrg

Cutting Depths

Start Depth (D) specifies the depth at which the V-Carving toolpath is calculated, allowing V-Carving / Engraving to be machined inside a pocket region. When cutting directly into the surface of a job the Start Depth will usually be 0.0. If the V-Carving / engraving is going to be machined into the bottom of a pocket or stepped region, the depth of the pocket / step must be entered. For example, to carve or engrave into the bottom of a 0.5 inch deep pocket, the Start Depth = 0.5 inches

Use Vector Start Points

If this option is checked ✓, the start point of the profile and offset toolpath segments will be as close as possible to the start point of the corresponding boundary vector. Otherwise this is left up to the program.

Toolpaths | Vector Selector

This tool allows you to easily select vectors which meet a set of criteria, such as open, closed, circular and also matching constraints based on layers. The dialog can be accessed from the Edit ► Vector Selector menu item, or from the button on each toolpath form. When the command is executed the dialog shown is displayed.

The dialog is used to configure a set of 'filters' that determine which vectors will be selected. A filter is enabled by clicking on its check box, or selecting a 'radio button' option, the current selection will be updated with all the objects in the file which match the current filter options.

Generally you will start at the top of the dialog and work downwards, specifying more and more explicit filters to determine the required selection exactly.

The simplest option is just to use the form to Select Closed Vectors in the job or Select Open vectors (you can specify both, in which case all vectors will be selected as long as they are on a visible layer).

The most common way to use the Vector Selector is to select all the vectors on a given layer as shown in the screenshot of the dialog below.

[object Object]
In this example, the dialog has been used to select All Closed Vectors on the layer with the name Pocket.

Note

When opened from Edit ►Vector Selector, the options Associate with toolpath and Set toolpath Cut Depth from imported vectors are not available. These options are only usable when applying the vector selector from a toolpath form.

Selection

The Selection: section at the top of the dialog is continuously updated to show the results of the current filter and the 2D view is also updated to show what is currently selected. The Objects: entry shows the total number of objects selected, if these objects include Text or Groups, this number may be less than the total of Closed and Open vectors displayed on the following line. For instance, a block of text is one object but will usually consist of many closed vectors. If a group contains both open and closed vectors, it will be selected as matching both Open and Closed filters.

Geometry Filters

The Geometry Filters section is used to specify constraints on the type of vectors to select. You can choose to select open vectors and/or closed vectors. Instead of selecting All Closed Vectors, the dialog can be used to select Only Circles and can even be used to specify an exact diameter and tolerance for the circles to be selected. This can be very useful for selecting vectors for drilling toolpaths, particularly if the vectors have not already been sorted into layers.

Layer Filter

The Layer Filter section allows you to pick one or more visible layers on which to select vectors which match the geometry filter. Alternatively, the All visible layers option disables the filtering by layer and selects all vectors which match the geometry filter regardless of the layer they are on, as long as that layer is visible.

Advanced Toolpath Templates

By associating a template with the result of a Vector Selector filter, we can make a template to automatically select the vectors it is intended to machine. A simple case would be to create a template which consisted of a Pocketing toolpath set up to machine all closed vectors on a layer called Pocket. After loading this template into a new job and choosing Toolpaths ► Recalculate All Toolpaths , the toolpath would be recalculated automatically selecting all closed vectors on the layer called Pocket.

The advanced templates are created by selecting the vectors for a toolpath using the Selector... button on the toolpath form. When a toolpath form is first opened, the Vector Selection: section on the form will show that vectors are being selected manually as shown below...

Pressing the Selector... button will display the Vector Selector form as shown previously. After making your geometry selection and before you close the form, select the Associate with toolpath option on the form as shown below.

After the Vector Selector form closes, the Toolpath form will indicate that Vector Selection is now 'Automatic' as shown below...

Note

Calculate the toolpath to apply the changes you have made.

When you re-calculate or edit a toolpath that has the Vector Selection mode set to automatic, the vectors which match the filter when the toolpath is re-calculated or edited will be selected. To cancel the Automatic vector selection mode, you can just select the vectors to machine normally with the mouse, or use the Selector... button to bring up the Vector Selectordialog again (the settings are remembered) and uncheck the Associate with toolpath option.

If toolpaths with the Vector Selection mode set to Automatic are saved as templates, these setting are saved with the template. When the template is re-opened and the toolpaths recalculated, they will automatically select all vectors which match the filters specified with the Vector Selector for that toolpath.

If you load a toolpath template which has toolpaths associated with layers which don't exist in the current file, the Missing Layers for Template dialog will be displayed. It lists all the missing layers and offers you the choice of having them created automatically, deleting toolpaths associated with missing layers or just loading the toolpaths as is.

Choosing to allow the dialog to automatically create the missing layers allows a toolpath template to be used to create 'standard' layers for machining operations and load the toolpaths ready to be calculated. All you then need to do is move vectors to the appropriate layers and recalculate all the toolpaths.

Choosing the Delete all toolpaths associated with missing layers option allows you to create a single template with many toolpaths and have the ones which aren't appropriate to the current job automatically deleted.

Preinstalled Gadgets | Celtic Weave Creator

This Gadget dramatically simplifies the creation of complex 3D Celtic weave patterns using an interactive interface to produce all the vectors required by the Extrude and Weave tool.

Using the Gadget to create the 2D Artwork

Knot Grid

Simply define the size of the weave grid you require. Click to see your changes reflected in the Weave Preview Image.

Weave Preview Image

Click on the interactive weave image to cycle through the different crossing options at each intersection point. The 3 options are:

  • Cut Vertical
  • Cut Horizontal
  • Cut Neither

You can reset the Weave Preview Image at any time using the button.

Cross Sections for Extrude

When you are happy with the layout of the weave pattern, choose which cross-section you would like and click to add it to your 2D View.

Click the button to convert the weave design you have created into vectors artwork in the 2D View. You can change the Weave Preview Image and click to update this artwork as often as you like.

Click once you are happy with your design. The Celtic Weave Creator form will close, but if you re-select the unedited weave pattern in the 2D View and re-open the Celtic Weave Creator gadget it will reflect you currently selected weave in the Weave Preview Image for further editing.

Preinstalled Gadgets | Create Rounding Toolpath

This gadget is used to simplify the task of creating toolpaths to machine a rough blank to a finished diameter for users with a rotary axis / indexer. It supports rounding from either round or square stock and creates the toolpaths directly from the gadget. The gadget is designed to be used in a rotary job

As with all Vectric gadgets, the first part of the form gives an overview of the gadgets purpose.

The start of the form also makes a VERY important point about where the Z origin should be set when the toolpaths are output via a wrapping post-processor. This has to be configured during job setup.

You have the choice of specifying if the tool is being zeroed on the center of the cylinder or the surface. When you are rounding a blank, you cannot set the Z on the surface of the cylinder, as the surface it is referring to is the surface of the finished blank. We would strongly recommend for consistency and accuracy that you always choose 'Center of Cylinder' when outputting wrapped toolpaths as this should always remain constant irrespective of irregularities in the diameter of the piece you are machining or errors in getting your blank centered in your chuck.

A useful tip for doing this, is to accurately measure the distance between the center of your chuck and a convenient point such as the top of the chuck or part of your rotary axis mounting bracket. Write down this z-offset somewhere, and zero future tools at this point and enter your z-offset to get the position of the rotary axis center

The Create Rounding Toolpath form is divided into 4 logical sections.

Blank Size and Shape

The gadget supports creating a toolpath to machine either a square blank or a round one. In this section you specify the shape of your initial blank and its dimensions. The diagrams show which dimensions are being specified.

Machining Method

The gadget offers a choice of three types of machining and for all types you can enter an allowance that will be left on the final shape if required. The Radial and Raster options can be used with either square or round blanks, the Optimized Raster can only be used for square blanks.

Radial (around cylinder)

This option creates a toolpath which rotates the blank around its axis 360° before stepping over to the next pass by the tool stepover distance and rotating the blank back again.

Raster (along cylinder)

This option machines along the length of the cylinder before incrementing the rotary axis round by an amount equal to the tool stepover and then returning the tool back along the cylinder axis. For many machines where the rotary axis is often slower than the X or Y axis, this strategy may allow shorter machining times.

Optimized Raster (along cylinder)

If you are machining a square blank into a round shape, the previous options generate a large number of wasted toolpath moves, because for much of the machining process they are machining 'fresh air'. The 'Optimized Raster' strategy only creates the toolpaths where there is actually material on the blank and hence is much more efficient for square stock.

After choosing your machining method, the next section on the form allows you to pick the tool you will be machining with. The tool is selected from the standard Vectric tool database and will control the stepover, step down and feed rates for the toolpath. It is important to note that after choosing the tool you will not be able to edit the parameters, so you must set up the tool with the correct parameters in the tool database to begin with. This section also allows you to specify a name for the toolpath which will be created.

The values in the final section of the form are picked up automatically and are presented for reference only.

After filling in all the values (all values will be remembered as the default values to use the next time the gadget is run), press the OK button and the toolpath will be generated within the program.

Preinstalled Gadgets | Drag Knife Toolpath

This Gadget supports drag knife tooling in your CNC machine. It uses the selected vectors in the 2D View as the basis of a centerline profile-type toolpath that incorporates swivel moves at corners to ensure the drag knife blade remains properly aligned throughout the cut.

Warning

When machining please ensure you have the spindle switched off.

Blade Offset

The tip of a drag knife is offset by a small amount from the pivot center of the tool to allow it to swivel as it cuts. This value specifies the distance and will be provided by your tool manufacturer.

Tolerance angle

This value determines when a swivel move needs to be used on a corner. Changes in tool direction, or corners, with angles less than this value will not generate swivel moves.

Cut Depth

This value sets the final cut depth of the toolpath. It defaults to be the current material thickness.

Swivel Depth

The knife must remain in some contact with the material in order to swivel correctly, but a small retraction is generally used to lift the knife blade slightly to minimize marking the material during the swivel action. This value must, therefore, be less than the cut depth and appropriate for your tool and material.

Passes

This value determines the number of passes used to cut down to full depth. The depth of each cut will be specified cut depth divided by the number of passes.

Use Vector Start Points

If Use Vector Start Points is checked ✓ then the gadget will use the existing vector start points to begin cutting vectors. Please note that this gadget assumes that the blade starts parallel to the positive x-axis. If this is option not checked the gadget will attempt to find what it thinks are sensible start positions.

Feed and Plunge Rates

These are the rates that the machine will push the knife through the material during a cutting pass, and the rate of descent of the tool into the material at the beginning of a cutting pass. Please ensure that the values are appropriate for your machine tool and the material you are cutting.

Preinstalled Gadgets | Job Setup Sheet Editor

The Job Setup Sheet Editor is a gadget which enables you to personalise the existing Job Setup Sheet that you can generate from the Toolpaths Menu. You can access the gadget from the Gadgets Menu.

Change Logo

To change the logo from the default Vectric logo, press the button. This will open a dialog box enabling you to search your local computer for images to select. Images in landscape are better suited as they will be scaled down to W165 x H52 pixels. Images must either be JPG, PNG or GIF file format.

Title

To change the default title of “Job Setup Sheet”, enter the desired title in the edit box.

Color options

There are two options to change the color of the Header and Footer blocks, you can either: Point and click the mouse in the colored edit box, this will bring up the color selector, select a color and then click anywhere outside of the selector to accept this. Type a colors hex value directly into the edit box.

Add or Remove Setup Sheet Information

Each of the 5 sections of the Job Sheet can either be included or removed to display as much information as required. The image to the left, represents a default Job Sheet which includes the following 5 sections:

  • Job Layout
  • Job Notes
  • Material Setup
  • Toolpaths Summary
  • Individual Toolpath Summaries

Restore to default sheet

Upon first successful run of this gadget, it will detect if you have already created a modified version of the Job Setup Sheet within the public gadgets directory, if so it will backup this Gadget so you could, if required restore it at a later date. If no modified gadget is found, it will backup the software default "Job Setup Sheet" so you have a copy if you want to revert back to the standard layout at a later date.

Preinstalled Gadgets | Keyhole Toolpath

This gadget simplifies the process of creating 'keyhole' toolpaths which are cut into the back of a sign or plaque to allow easy hanging on a wall. These slots are cut using a 'keyhole' cutter as shown on the left. The toolpath for these slots needs to plunge into the material at the mounting screw entry point to a depth that will ensure that the wide part of the cutter is below the material surface. The tool then moves along the 'slot', once it reaches the end of the slot, the tool retraces its path back along the slot to retract at the original plunge point.

Like all Vectric Gadgets, the top of the form gives brief instructions on how it should be used. For this gadget, you need to select one or more circular vectors in your design to indicate where you want the entry points for the keyhole slots to be before the Gadget is run. If you start the gadget without selecting one or more vectors to indicate these positions, the following warning will be displayed:

Once the form is displayed you can enter the parameters for your keyhole toolpath.

The data to be entered falls into three separate categories.

Slot Parameters

In this section of the form you specify the direction the slots will be machined and also the depth and the length for the slots.

Preview Drawing

To help with visualisation of the slot, the gadget can draw a vector outline of how the slot will appear on the surface of your job. This drawing is optional and if you un-check the Create Preview Vectors for outline on surface check box you do not need to fill in the parameters in this section. If you do want previews drawn, you can specify the entry hole diameter which will be created by your keyhole cutter and also the diameter of the slot the tool will create on the surface. You can also specify the name of the layer the vectors will be created on.

Toolpath Parameters

The final section of the form is used to specify a tool which the feed and plunge rates are picked up from, and also a name for the toolpath which will be created. As keyhole cutters are not supported natively by the program, just set up an end-mill with the required feed rates to use.

After entering all your parameters and pressing , the gadget will create a toolpath within the program to machine your slots and also the vector preview if you enabled this option. The screen shot below shows the preview vectors in the 2D view along with the toolpath in the 3D view.

Preinstalled Gadgets | Wrapped Fluting Layout

This gadget is used to simplify the task of creating toolpaths to machine flutes and coves on a rotary work piece. The gadget is designed to be used in a rotary job

This gadget does NOT create toolpaths directly. It lays out vectors in the 2D view which can then have toolpaths created using either the Profile or Fluting toolpaths within the main program. The top part of the form allows the user to specify how many flutes to create and how far from the start and end of the work piece the flute should start and end. Flutes are laid out evenly spaced based on the circumference of the cylinder. If the user chooses to create coves at either or both ends, extra vectors will be created which can be machined with the Profile toolpath and the Machine Vectors On option to create the coves.

The bottom section of the form contains details about the cylinder dimensions and is presented for reference only.

After the gadget has run the vectors required for machining will be visible in the 2D view. If you have a 3D form for your rotary piece, you can use the Project toolpath onto 3D model option on the toolpath forms to have your fluting toolpaths follow the work piece surface.

Preinstalled Gadgets | Wrapped Spiral Layout

This gadget is used to simplify the task of creating toolpaths to machine spirals (rope or barley twist) on a rotary work piece. The gadget is designed to be used in a rotary job

This gadget does NOT create toolpaths directly. It lays out vectors in the 2D view which can then have toolpaths created using Profile toolpath within the main program. The top part of the form allows the user to specify how many strands to create and how far from the start and end of the work piece the strands should start and end. Strand ends are laid out evenly spaced based on the circumference of the cylinder. The spacing between strands during spiralling can be controlled using either Spiral Pitch or Spacing between strands option. It is also possible to choose between right and left hand twists.

If the user chooses to create coves at either or both ends, extra vectors will be created which can be machined with the Profile toolpath to create the coves.

For machining both spirals and coves, Machine Vectors On option should be used.

The bottom section of the form contains details about the cylinder dimensions and is presented for reference only.

After the gadget has run it will display message saying how many revolutions will each strand made and the vectors required for machining will be visible in the 2D view. Please note that the vectors will be extending beyond the 2D boundaries of the job. That is expected and thanks to wrapping feature will end up producing spirals. Please refer to Spiral toolpaths

Modules | Laser Module

Note

The Laser Module extends the functionality of VCarve or Aspire and is currently only available to selected BETA testers while in development. This documentation is provided to support this testing process and this notice will be removed once the module is available for purchase. Please note: The Laser Module has been created and tested for use with OptLaser or J-Tech laser retrofit kits on Shapoko and X-Carve CNC machines using GRBL controllers - other machines, lasers or controllers cannot be supported at this time.

The Laser Module is a paid add-on for Cut2D Pro which adds the following additional functionality:

  • The ability to create Laser Cut and Fill Toolpaths
  • The ability to create Laser Picture Toolpaths
  • The ability to simulate a Laser Toolpath

The Laser Cut - Fill Toolpath

Laser Cut - Fill Toolpath is used for cutting out shapes or marking areas.

Cut-outs can take into account the kerf, or width, of the laser beam to maintain the precise internal or external size the selected vector shapes. Shapes can also be filled with stripes or hatching to create simple shading effects.

The Laser Picture Toolpath

The Laser Picture toolpath uses the laser and through varying the power of the laser etches a copy of the selected bitmap onto the surface of your material.

Simulating Laser Toolpaths

Like all other toolpaths the laser toolpaths can be simulated. However, in the case of laser toolpaths, the simulation does not remove any material but instead marks the surface of the current simulation model. This marking is meant to simulate the charring of the material when scorched by the laser.

Burn Rate 50
Burn Rate 50
Burn Rate 100
Burn Rate 100
Burn Rate 200
Burn Rate 200

Due to the many combinations of laser, power, material and feed rate, it will be necessary to calibrate the simulation so that the simulation output matches the real-world results. This calibration can be done by modifying the Maximum Burn Rate property of a given tool. This is the maximum speed at which the tool, when at 100% power, will still burn the material. This means that a greater value will result in the simulated toolpath appearing darker. This value can be set in the Tool Database. We suggest you cut a sample file with the material and power settings that you would typically use and then adjust the Maximum Burn Rate so that the simulation matches your achieved results.

Modules | VTransfer

VTransfer is a small helper application provided by Vectric to simplify the process of sending toolpaths to some Grbl-based controllers. You should run VTransfer on the PC which your CNC machine is connected to via a USB serial connection.

If your Vectric CADCAM software is also running on the same PC, you can use Direct Output mode to send toolpaths to VTransfer directly from the Toolpath Saving form, without the need for file saving or loading.

VTransfer also provides the commands you need to initiate basic homing, jogging and setting of origins on your CNC machine before a toolpath is run.

Controllers

VTransfer has been created specifically for streaming toolpaths to a pre-configured controller. It expects that your controller is correctly set-up and tested for your hardware. VTransfer will not set, alter or validate your controller's parameters in any way and is not intended to be used for lower-level controller configuration.

Getting Started

Before starting VTransfer, you need to ensure that your machine is powered on, any required drivers are already installed and the machine is accessible via a serial port (COM port on Windows). For most machines connected by USB, you will need to have installed the appropriate device driver for your machine controller. These drivers will be provided by your machine tool supplier and you should verify that your CNC machine connects correctly to your PC before attempting to use VTransfer.

When the machine and drivers have been installed correctly, refreshing and checking the drop-down Connect On: list will show your machine tool controller. VTransfer will still need to know the specific communication protocol required though and the first time you use VTransfer you will need to complete some one-time set-up and configuration.

Once set-up for a machine that remains connected to the same USB port of your PC, VTransfer should automatically detect and connect each time it starts-up.

Initial Set-up

Once this initial set-up has been completed, VTransfer should automatically detect and connect to your machine on start-up, provided the machine remains connected to the same USB port of your PC. Before connecting to your machine for the first time, however, you should complete the following steps to set the right controller type and maching configuration.

  • Select File->Settings from the main menu to open the Settings
  • Make sure that your controller is selected in the Controller Name: drop down list (for a Grbl version 1.x controller this will be Grbl, for example)
  • Select the correct configuration file for you machine, or create your own.

Controller Connection

  • Make sure that your machine is connected to the PC via USB and it is powered on
  • Click the button, regenerate the Connect On: drop down list with all of the detected devices connected to your PC.
  • Select your controller device from the list - note that this may be the name of the microcontroller on which your controller is running, rather than the controller name itself (grbl may appear as Arduino UNO, for example)
  • Check that the Machine Status reported by VTransfer reads Looking for... followed by the expected controller name
  • Machine Status will change to Connecting while VTransfer attempts to verify the controller is communicating as expected
  • Once correct communication has been established the Machine Status will change to Initialising, Alarm or Ready depending on how your machine is configured

Running a toolpath

Once connected to your CNC machine, the typical steps for running your first toolpath using VTransfer are:

  • Open the Jog Tab
  • If your Machine Status is Locked, either or Unlock your machine (if supported and configured)
  • Load your toolpath file or send one to VTransfer via Direct Output
  • If required, jog the machine to the location of the material on your CNC machine (to match the relative origin point of your toolpath) and set the
  • Fit the required tool
  • Either run the Z Touch Plate cycle (if supported) to set Z Zero to match your toolpath
  • Or manually jog the tip of the tool to the material surface or machine bed (again to match the Z Zero setting of your toolpath) and set the
  • Ensure the spindle is on (if it is not controlled automatically)
  • Open the Cut Tab - Click

Sending a toolpath directly to VTransfer from your Vectric software

At the point of saving your toolpath some post-processors support the option of Direct Output to VTransfer (such as the Emblaser or X-Carve). If you have one of these post-processors selected, the Output direct to machine checkbox will be enabled below the post-processor selection box in the Toolpath Saving form.

With this box checked, will change to and clicking this button will automatically send the toolpath to VTransfer. If VTransfer is not already running, it will launch automatically.

Whenever a new toolpath is loaded or received by VTransfer it will prompt you with a message box.

Homing, Jogging and Origins

Before running your toolpath, it is essential to set your machine's origins appropriately. The specific process you need to use will, to a large extent, will be determined by your machine and its configuration. Generally you will need to home your machine (if supported) and set the X Y origin to match the intendended toolpath and location of the material on your machine's bed. You will also need to fit the correct tool and typically set the tip of this tool to be at Z Zero, either at the top or bottom of your material - again this choice will already have been determined when your toolpath was created. The commands relating to these actions are all available from the Jog tab.

Whenever VTransfer changes its origin settings you will be prompted with a message box.

Start Homing Sequence

Click this button to initiate the homing sequence. The homing sequence will culminate in setting the origins of your machine using its homing switch locations and the machine's machineable area - both of which are set in the configuration. For some controllers (such as Grbl) you will typically be required to run this command before you can do anything else because the machine will start-up in a disabled Alarm status.

Note

This button is only available if your machine is configured with homing switches and homing is enabled.

Z Touch Plate

This button will be visible if your machine is configured with a touch plate, touch plate support is enabled and its thickness is set in the configuration settings. Click it to initiate the Z touch plate probing cycle. Make sure that the touch plate is in position and correctly functioning before clicking this option as it will immediate begin a plunge move.

Warning

Make sure that the touch plate is in position and correctly functioning before clicking this option as it will immediately begin a probing plunge move.

Jogging

The , , , , and buttons will each jog the machine along the Y, X or Z axes, respectively.

The distance moved by each button click is determined by the current value (in mms) shown in the drown-down control at the center of the jogging buttons. Ensure that you adjust this value appropriately before using the jog buttons to move the machine.

Lasers

If the selected configuration for your machine has a Z travel value of zero, this indicates that the machine does not have a Z axis - this is the case for most laser cutters - and Z axis controls will not be visible.

Setting and Resetting Origins

By default a machine with homing support will have its X Y origin (the postion of the coordinate X:0 and Y:0) set to the bottom left corner of machine's machinable area following a homing cycle - i.e. the machine will operate in a positive coordinate work space within its machinable area. For machines without homing support, the initial X Y origin must alwaysbe set manually before running a toolpath. In additon, when a toolpath is created it is very common that the X Y origin will actually be chosen to be relative to the material (not the machine bed) - for example, the center of a design may be used. For most toolpaths, therefore, you will need to jog the machine to the matching origin location for the toolpath (relative to your material), and manually before cutting.

For machines with homing support, you can restore the bottom left corner origin after setting it for a specific toolpath by clicking at any time. When this button is clicked the location of coordinate position X:0, Y:0 will once again be set to the bottom left corner of the machine's machinable area.

Running the Toolpath

The Cut tab contains the controls need to begin cutting your toolpath and monitoring its progress.

Cut Now

When your machine is correctly set-up (with the X,Y and Z origins set), click this button to begin streaming the toolpath to your machine and begin cutting.

Warning

Make sure your machine spindle is on before clicking this button if your spindle control is manual.

Estimated Time Remaining

Once your toolpath has started, VTransfer will provide a dynamic estimate of the remaining time until the toolpath is finished.

Dynamic Feedrate Override

If your machine supports feedrate override control and the option is enabled in your configuration, then the and buttons will be available. Click these buttons to increase or decrease the current toolpath feedrate by 10%. The current state of the feedrate override setting is indicated by the percentage value between the two control buttons.

Delay

Depending on the nature of the toolpath you are running, there may be a delay of one or more seconds before your machine responds to the feedrate change so allow for this when using these controls.

Abort

This button will stop the toolpath as quickly as possible, usually resetting the controller in the process. Once a toolpath has been aborted you should re-home and re-origin before running a subsequent toolpath.

User Guides | 2D Design and Management

he 2D View is used to design and manage the layout of your finished part. Different entities are used to allow the user to control items that are either strictly 2D or are 2D representations of objects in the 3D View. A list of these 2D View entities are described briefly below and more fully in later sections of this manual.

Ultimately the point of all these different types of objects is to allow you to create the toolpaths you need to cut the part you want on your CNC. This may mean that they help you to create the basis for the 3D model or that they are more directly related to the toolpath such as describing its boundary shape. The different applications and uses for these 2D items mean that organization of them is very important. For this reason Aspire has a Layer function for managing 2D data. The Layers are a way of associating different 2D entities together to allow the user to manage them more effectively. Layers will be described in detail later in the relevant section of this manual. If you are working with a 2 Sided project you can switch between the 'Top' and 'Bottom' sides in the same session, enabling you to create and edit data on each side, and using the 'Multi Sided View' option you can view the vectors on the opposite side. 2 Sided Setup will be described in detail later in the relevant section of this manual.

Vectors

Vectors are lines, arcs and curves which can be as simple as a straight line or can make up complex 2D designs. They have many uses in Aspire, such as describing a shape for a toolpath to follow or being a controlling 2D shape for use with one of the 3D modeling functions such as the 2 Rail Sweep. Aspire contains a number of vector creation and editing tools which are covered in this manual.

As well as creating vectors within the software many users will also import vectors from other design software such as Corel Draw or AutoCAD. Aspire supports the following vector formats for import: *.dxf, *.eps, *.ai, *.pdf, *skp and *svg. Once imported, the data can be edited and combined using the Vector Editing tools within the software.

Bitmaps

Although bitmap is a standard computer term for a pixel based image (such as a photo) in *.bmp, *.jpg, *.gif, *.tif, *.png and *.jpeg. These file types are images made up of tiny squares (pixels) which represent a scanned picture, digital photo or perhaps an image taken from the internet.

To make 3D models simple to create, Aspire uses a method which lets the user break the design down into manageable pieces called Components. In the 2D View a Component is shown as a Grayscale shape, this can be selected and edited to move its position, change its size etc. Working with the Grayscale's will be covered in detail later in this manual. As with bitmaps, many of the vector editing tools will also work on a selected Component Grayscale.

User Guides | 3D Design and Management

As well as creating toolpaths directly from 2D drawings, Aspire can produce extremely flexible 3D toolpaths. These toolpaths are created from 3D design elements called 3D Components that can be generated from models created in external 3D design packages , imported as 3D clipart or built entirely from within Aspire using 2D artwork as a source.

The 3D View

The 3D View can show you the current Composite Model

The Composite Model

Aspire has been designed to work in a way which enables the user to easily create even very complex projects. In any situation, the best approach to producing something complicated is to break it down into smaller pieces until a level of simplicity is reached that can be understood and managed. In Aspire this is achieved by letting the user work with pieces of the design which are combined to make the finished part. In the terminology of the software these pieces are called Components. To help organize the Components they are assigned to Levels. Step by step, Components and Levels can be created and modified until you have all the elements you need. In the images below you can see an example of how this might work. On the left you can see the separate component for a model of a bunch of grapes and on the right you can see these positioned to make the complete part - we call this resulting combination the Composite Model.

There is no limit to how simple or complex a Component or the Components on a Level can be (this is the user's choice). In the example shown, you can see that a model of a whole bunch of grapes may be made up of smaller individual components but they could also be combined to exist as one single Component (the assembled bunch of grapes) that could then be used to lay-out a more complex part with multiple bunches of grapes. They could also be organized so all the grapes were on one Level and leaf and stem on another to provide a different way of managing and manipulating the shapes. Each user will find a level of using Components and Levels they are comfortable with which may be dependent on the particular job or level of proficiency with the modeling tools.

3D Components and Levels

In Aspire, the aim is to end up with a set of Components and Levels that when combined together will make the finished 3D part. One way to think of this is like building a 3D collage or assembly. As the design evolves, new Levels or shapes may need to be created or existing ones changed. The parts of the collage are managed with the Component Tree

Creating and Editing Components

An existing Component can be copied, scaled and have other edits carried out on it as an object. The user can also change the way it relates to the other Components, for instance whether it sits on top or blends into an overlapping area of another Component. The shape, location and relation of these pieces determine the look of the final part. As the job progresses, the user will need to create brand new Components or edit existing ones by adding new shapes, combining them with others or sculpting them.

Components can be created and edited by:

  1. Use a modeling tool to create shapes from 2D vectors.
  2. Import a pre-created 3d model - either a model previously created in Aspire or from another source such as a clipart library or a different modeling package.
  3. Create a 'texture' Component from a bitmap image.
  4. Use the Split Components Tool to break an existing Component into multiple pieces.

All of these methods are covered in detail throughout the training material.


Dynamic Properties

As well as having its underlying 3D shape, each component also has a number of dynamic properties that can be freely modified without permanently changing its true shape. These include scaling of the Component's height, the ability to tilt it, or to apply a graduated fade across it.

These dynamic properties can always be reset or altered at any time during your modeling process, which makes them a particularly useful way of 'tweaking 'your components as you combine them together to form your final composite model.


Combine Modes

The Combine Mode is a very important concept when working with 3D shapes within Aspire. The options for combine mode are presented when creating new shapes and also when deciding how Components and Levels will interact in the Component List. Rather than cover this in every section where it is applicable, it is worth summarizing the options here so the general concept can be understood.

When you have more than one 3D shape, such as the Component pieces of the design or where you have an existing shape and are creating a new one, then you need to have a way to tell the software how the additional entities will interact with the first. This can be an abstract concept for users who are new to 3D but it is an important one to grasp as early as possible. In Aspire this is controlled by a choice called the Combine Mode.

There are four options for this: Add

As modeling is an artistic and creative process, there is no general rule to describe when to use each one. As a guide though you can assume that if the second shape's area is completely within the originals one then you will probably be adding or subtracting and if the shapes only partly overlap that you will probably use Merge or, very occasionally, Low.

The four options and their specific effects are described on the following pages. To illustrate the different effects a combination of an overlapping beveled square and a dome will be used. You can see in the image top right how these are arranged in the 2D View and how they overlap. Then you can see each individual shape in the images below middle and right. These shapes will be used to demonstrate the different Combine Modes. In every case the Dome will be considered the primary shape and the square is the secondary shape which is being combined with the first. In addition to the dome/square example some images of 'real world' parts will also be included to help to understand how these can be used on actual projects.

As well as working on individual shapes, the Combine Modes are also assigned to Levels. These will govern how the combination of all the individual components on one Level interacts with the result of all the Components on the Level below it in the Component Tree

Note:

There is a 5th Combine Mode available from the right mouse click menu after a component has been created called Multiply. This combine mode has specialist applications which are dealt with in the appropriate tutorial videos. This option will literally multiply the heights of the Component or Levels being combined to create the new Composite 3D shape.

Add

When Add is selected, it takes the first shape and then just adds the height of the second shape directly on top of the first. Any areas which overlap will create a shape which is exactly the height of each shape at that point added together (see below)

Typically the add option is mainly used when the shape being added sits completely within the original shape, this ensures that the uneven transition where the parts only partly overlap (as shown in the example) do not occur.

The example above shows the Maple Leaf and border extrusion Components being Added to the dome Component in the sign example from the Introduction to Modeling document.

Subtract

When Subtract is selected it takes the first shape and then removes the height of the second shape from the first. Any areas which overlap will be a combination of the original height/shape less the second shape. Areas where the shape goes into the background will become negative regions. You can see how this looks using the dome and square in the image below:

Typically subtract, like the add option, is mainly used when the shape being removed sits completely within the original shape, this ensures that the uneven transition where the parts only partly overlap (as shown in the example) do not occur.

The image shown above has some 'creases' to help define the muscles of the lioness. The shapes to create these recesses were created by using the Subtract option with the Create Shape tool on the vectors representing those recessed areas.

Merge

When the Merge option is selected any areas of the shapes which do not overlap remain the same. The areas that overlap will blend into each other so that the highest areas of each are left visible. This results in the look of one shape merging into the other and is in effect a Boolean union operation. You can see how this looks using the dome and square in the image below:

Typically the merge option is used when the shape being combined partly overlaps the original shape. This enables a reasonable transition to be made between them.

The image above shows 2 Herons, a rope border and banner Components. Each of these overlaps with the others and so they are set to Merge in this areas. Whatever is the higher of the two merged areas is what is prominent. In this case the rope is lower than everything and the Banner is higher than the Herons so the desired effect can be achieved.

Low

The Low option is only available when combining Components (not in the modeling tools). When this mode is selected, any areas which do not overlap are left as they were in the original two shapes. Any areas which overlap will create a new shape which is the lowest points taken from each shape, this is in effect a Boolean intersection operation. You can see how this looks using the dome and square in the image below:

The Low option is used for recessing a shape into a raised shape. An example of this is shown in the image above.

The example shown on the right above uses the Low option to combine the flat topped 'button' component on the left with the curved top face component with the letter 'A' on the right. Combining both components with the merge low option gives the keyboard button with the curved top you see in the bottom row.

Level Mirror Modes

Right-clicking Levels in the component tree will open a pop-up menu offering commands and operations related to the clicked level and Mirror Modes can be set in this way. If a mirror mode is set on a Level, all the components it contains will be continually mirrored dynamically as they are moved, transformed or edited. The mirroring is non-destructive, that is it can be turned off or on at any time and does not alter the underlying components in any permanent way. Working inside a Mirror modes Level is a simple way of achieving a complicated symmetrical pattern by editing only one half (or quarter, see below) of the design.

The available Mirror Modes are broadly divided into two groups. The first group apply one plane of symmetry:

  • Left to Right
  • Right to Left
  • Top to Bottom
  • Bottom to Top

These modes allow you to work in one half of your job and the other half will be automatically and dynamically generated for you. For example, in Left to Right mode you would place your components in the left half of your job and a mirrored equivalent of each would be created in the other half of the job. This 'reflection' is updated dynamically as you work.

The other group offer two planes of symmetry (horizontal and vertical):

  • Top Left Quadrant
  • Top Right Quadrant
  • Bottom Left Quadrant
  • Bottom Right Quadrant

When using these modes your components should all be in the quadrant (quarter) of the job. Mirrored reflections horizontally and vertically will be created in the other quadrants of the job for you.

Multi Sided View

When working in a 2 Sided environment you can create components independently per side or using the Right click option you can copy or move a component to the opposite side. Selecting the option to work in 'Multi Sided View' allows you to view components you may have on the Top and Bottom side in the 3D View. In the Toolpath Preview form of a project that contains toolpaths for the Top and Bottom Sides the multi sided view presents the simulation of the toolpath preview on both sides also, if the multi sided view is not selected you can use the 'Preview all Sides' option in the Toolpath Preview form to display the Top and Bottom Toolpaths in the 3D view. 2 Sided Setup will be described in detail later in the relevant section of this manual.

User Guides | 3D Toolpath Files

Files from Vectric's Cut3D, PhotoVCarve and Design and Make Machinist that include 3D toolpaths can be imported into Cut2D Pro using the main menu command: File ► Import ► PhotoVCarve, Machinist or Cut3D Toolpaths.

The 3D file must first be scaled to the required size before toolpaths are calculated, and then the complete file saved ready for importing into Cut2D Pro. These files can only be moved and positioned inside Cut2D Pro but cannot be scaled.

A Grayscale thumbnail of the 3D job is drawn in the 2D View with the X0 Y0 origin at the position it was set in Cut3D, PhotoVCarve or Design and Make Machinist. The associated toolpath(s) are also drawn in the 3D window and the names appear in the Toolpath list.

Positioning

To move the 3D design toolpaths open the 2D Window, click the Left mouse Twice on grayscale image (turns light Blue to indicate it's selected), then drag to the required position, or use the Move or Alignment tools for accurate positioning.

The toolpath(s) are automatically moved in the 3D window to the same XY position as the image.

Origin for the 3D data at X0 Y0
Origin for the 3D data at X0 Y0
Grayscale image moved to middle of job
Grayscale image moved to middle of job

Toolpaths for the example above have been calculated with the X0 Y0 in the middle of the 3D design. When imported into Cut2D the data is automatically positioned using the same coordinates, which places three quarters of the design off the job. In the second image the grayscale image has been moved to the middle of the job.

The 2D mirror and rotate drawing tools can also be used to edit the 3D data set.

3D toolpaths can also be copied using the Duplicate Toolpath command on the Toolpaths Tab making it very easy to use multiple elements from a single design on a job. The thumbnail preview is also copied for each toolpath, making it very easy to position additional copies of a 3D toolpath.

For example, a single design can be copied and mirrored to create Left and Right versions of a 3D design or to place multiple copies of a decorative design in the corners of a cabinet door panel as shown below.

[object Object]
The 4 corner roses are all copied from a single file

Toolpaths for the 3D elements can be previewed along with the conventional Profile, Pocketing and Drilling toolpaths, and everything will be saved ready for machining.

A good example of where this functionality might be used in conjunction with PhotoVCarve is for making personalized picture frames that include the PhotoVCarve grooves plus descriptive engraved text and a decorative Profiled or Beveled border. As shown below:

2D window showing thumbnail previews, text and decorative border
3D window previewing the completed job

Options

Imported toolpaths can also be edited to position them inside the material or to change the cutting parameters - speeds and feed rates can be changed.

Design and Make Machinist

When using a Design and Make Machinist file that includes multiple toolpaths, you must remember to edit the Start Depth for all of the imported 3D toolpaths.

Click the Edit toolpath icon or Double click on the toolpath name to open the edit form.

For example, after machining a half-inch deep pocket a PhotoVCarve design can then be edited to have a Start Depth = 0.5 inches and this will carve the photograph onto the base of the pocket surface.

User Guides | Advanced Modelling of 3D Rotary Projects

Modelling 3D spiral features

A column with a spirally wrapped design

In this section we will show how to use level-wrapping feature to wrap a design in spiral manner around a column.

The workflow for creating spiral toolpaths has been presented in Simple rotary modelling using 2D toolpaths chapter. The basic idea involved creating a line at a proper angle to the rotation axis, that exceeded the 2D boundaries. When 2D toolpath is created based on such a line, it will be wrapped around material cylinder, creating a spiral.

This guide will build on that basic idea. The task is to create a horizontal strip with desired pattern and then wrap it like a ribbon around the cylinder.

To help with that task, it is important to create some helpful vectors first. We need to create lines, that will become boundaries of our strip. In this example the strip was being wrapped four times around full length of material. This example assumes that rotation axis is parallel to X axis.

To start, select Draw Line/Polyline tool and draw a horizontal line at the bottom of the job from left to right. If it is desired for the spiral pattern to only fill part of the cylinder length, this horizontal line should be drawn only in th desired location. While the drawing tool is still active, type 90 into Angle box and type y * 4 into Length box and pressing =. We used y * 4 formula so the strip will wrap 4 times. Then press Add button to add a vertical segment.

Now, start a new line that connects the horizontal and vertical lines, forming a triangle. Once this line is created, horizontal and vertical lines can be removed.

The line that we just created will form a bottom of the strip. Now copy this line and place line so its bottom left end coincides with top left corner of 2D job. This line will form a top of the strip. Then make another copy and place it in the middle. This middle line will be used later to position our design within strip. All three lines have been shown below.

Next step is to find out the required length and width of the strip. We will need a few extra vectors to accomplish that.

Let's copy one of the created three lines and rotate by 90 degrees, to get a line that is perpendicular to the strip. Then place it in such way so it crosses the strip. This will help us measure the width.

Then copy the perpendicular line and place it so it touches the top line. Then extend the bottom line, until it crosses the perpendicular line we just added. This will help us measure the length of the strip.

Easiest way to achieve that, is to create a textured component. To do that, select the design in the component tree and activate the Create Texture Area tool. This example used the default settings of the tool. The tool will create a new component that will fill the whole 2D job boundaries. The component itself will be filled with the design in tiled manner. Now use Set Size tool to resize textured component to match the strip size.

Now the component have to be rotated and moved to fit between the lines be have drawn at the beginning. This process can be made easier by utilizing Copy Along Vectors tool. To proceed, activate the tool and select the textured component first, then select the middle line in the strip while holding Shift. Make sure that Align objects to curveoption is selected and use Number of copies option. Since our strip has already have a correct size, we only need one copy. However the tool would place the middle of our component at the beginning of the line only. If enter 3 as the number of copies, then the tool will place two copies of component at each end and in the middle. Afterwards copies at the ends can be simply deleted. The picture below shows the strip in the 3D view after being correctly positioned.

As can be seen, the strip disappears as soon as it leaves the material boundaries. In order to make it wrap around, we need to create a new level in the component tree and move the texture component into it. Then right click on the newly created level and right click. From the pop-up menu select wrapping. After that wrapping will occur.

Note:

Wrapping can be enabled on any level in component tree and combined with mirror mode. If the level wraps on itself, then intersecting areas will be merged regardless of level's combine mode. If it is desired to create e.g. a woven pattern, then place left-hand spiralled component and right-hand spiralled components in different separate levels, both with wrapping enabled.

The last step is to make column endings. For that purpose third level was created, with Combine Mode set to Merge. This way the spiral pattern will be 'hidden' at the ends. A circular 3D tab clipart was placed at each end, and stretch vertically to match the job boundaries.


Modelling twisted shapes

A twisted star

This section will show how to create twisted shapes, using combination of level-wrapping and Vector Unwrapper tool.

In this example a new rotary job was created, with diameter of 6 inches and length of 20 inches, rotating around X axis. To start, we need a cross-section vector. In this example a 5-armed star was used. To create a star, we can use Draw Star tool. This example used Outer Radius of 3 inches, to match the radius of the material.

The next step is to unwrap the cross section. In the case of star however, the center is not the same as center of star's bounding box. To find the real center, one can draw line from two of the star corners. Then open Vector Unwrapper and select the star. Then drag rotation center and snap it to the intersection of the lines, as can be seen below.

Using Vector Unwrapper with the star-shaped vector
Rails and uwrapped star


Once the star is unwrapped, we need to create rails, that will make spiral when wrapped. To do that, select Draw Line/Polyline tool and draw a horizontal line at the bottom of the job from left to right. While the drawing tool is still active, type 90 into Angle box and type y * 2 into Length box and pressing =. We used y * 2 formula so the star will make 2 revolutions Then press Add button to add a vertical segment. Finally, start a new line that connects the horizontal and vertical lines, forming a triangle. Once this line is created, horizontal and vertical lines can be removed.

Next step is to copy the line and place it so its bottom left end coincides with top left corner of 2D job.

Once the the rails are ready, one could use a Two Rails Sweep tool. However, since rails exceeds the 2D job boundaries, the created sweep will be cropped as soon as those boundaries are exceeded.

To overcome that, select both rails, open Draw Rectangle tool and press Create. This will create a bounding box containing the rails. Now, write done the size of the box and save current project. Then create a new single-sided project with the slightly bigger than the bounding box. Use Import Vectors option from the main menu and select previously selected file. Now select the rails and press F9 to center them.

Now use Two Rail Sweep tool. When component is ready, save the file.

Now re-open the original rotary project. Use Import Component and select single-sided project created in the step above. Move the component to the desired location. Then, create new level, move the component there and enable wrapping.

Using single-sided modelling tools

A table leg modelled using techniques from single-sided modelling

This section will present how to use single-sided modelling techniques in rotary projects.

Users familiar with modelling techniques used in single-sided projects may find them more convenient for modelling certain shapes. This example uses two vectors, representing side cross section of the table leg and a few of half cross sections for different parts of the table leg. Those vectors are presented below.

Various cross sections of the modelled table leg

One can simply treat side cross section as rails and use Two Rail Sweep tool, placing half cross sections at appropriate locations. This way half of the leg can be modelled very quickly, with the result that can be seen below (using flat 3D view).

Flat 3D view of modelled half leg

In order to use the created model in rotary project, we need to export and then import it back. Although it is possible to do this with two sessions of Aspire, it can also be done within a single session with rotary project. To export the leg model, make sure no other components are visible (including the automatically added zero plane) and open Export Model tool while holding down Shift. Pressing Shift allows to open the export tool in single-sided, rather than rotary mode.

Since half of the leg was modelled, Close with inverted front option was used. The resulting STL mesh can be seen below.

STL model of the leg to be exported

Once component is exported, it can be re-imported as Full 3D model. The model wil have a seam, in the place were two halfs were merged. This can be removed using smoothing function of Sculpting tool.

User Guides | Crash Handling

In the unfortunate event of the software crashing,

  1. We try to save unsaved changes, so that your data isn't lost.
  2. Provide an easy way for you to report the crash so that we can work on a fix.

Project Saving

If you're working on a job and the software crashes, the first thing it will try to do is to save your project. The project will be saved alongside your original to avoid accidentally corrupting your original file.

Report the crash

A dialog will pop up asking you to upload the crash information which will help us track down the issue. Any information you can think of would be greatly appreciated and will help us fix the issue in a timely manner.

Description

Please try to remember what you were doing at the time, and describe it for us. Please include any information you can think of. Any bit of information can help us track the issue quicker, so we greatly appreciate that.

Information

You can include your name and e-mail to allow us to get back to you with questions in case we need more information. For example, we may need the project that you were working on. This data will not be used for any purpose other than to help us track down the issue.

Internet

You will need to be connected to the internet for this to work. If not, you can still send the generated zipped report to support@vectric.com. The report can be found in the Application Program Data (Accessible through the menu FileOpen application data folder.... If you try to send the report and it fails, you will get a message of where that path is and possible methods to get that report to us.

The crash reporting is powered by BugSplat (a third-party) company which provides us with the tools that help us analyse them.

User Guides | Creating a Rotary Job

XY Origin

XY Drawing Origin - Here you can specify where the XY zero origin will be placed on your job. These options correspond to the same fields on the normal 'Job Setup' form within the program. Most people would use the default Bottom Left Corner, but for some jobs you may prefer to have the XY origin in the Center.

  • In a job with horizontal orientation (Along X Axis), the X offset will correspond to the length of the cylinder, and the Y offset will be a point along its circumference.
  • In a job with vertical orientation (Along Y Axis), it's the opposite. The Y offset will correspond to the length of the cylinder, and the X offset will be a point along its circumference.

Orientation

Cylinder Orientation Along - This section is used to tell the program how you have your rotary axis aligned on your machine. If you've already made your design, but just want to change the job for a different machine, then you could flip your design with the material so that all the vectors and components stay the same relative to the job.

Z Origin On - This section determines whether the Z Origin is set to the surface of the material or the base (center of cylinder). These settings can be over-ridden when the toolpath is actually saved, but we would strongly recommend the 'Cylinder Axis' is selected for rotary machining. The reasons for this are detailed in the note below.

Z Origin

You have the choice of specifying if the tool is being zeroed on the center of the cylinder or the surface. When you are rounding a blank, you cannot set the Z on the surface of the cylinder, as the surface it is referring to is the surface of the finished blank. We would strongly recommend for consistency and accuracy that you always choose 'Center of Cylinder' when outputting wrapped toolpaths as this should always remain constant irrespective of irregularities in the diameter of the piece you are machining or errors in getting your blank centered in your chuck.

Tip:

A useful tip for doing this is to accurately measure the distance between the center of your chuck and a convenient point such as the top of the chuck or part of your rotary axis mounting bracket. Write down this z-offset somewhere, and zero future tools at this point and enter your z-offset to get the position of the rotary axis center. Another reason for choosing 'Center of Cylinder' is that some controls will be able to work out the correct rotation speed for the rotary axis based on the distance from the center of rotation. If the Z value is relative to the surface, the control would need to know the diameter or radius of the cylinder at Z zero.

Vector Layout

As well as creating a job at a suitable size for wrapping toolpaths, when creating the job, it will create a number of vectors which can be very useful when creating your wrapped job.

The vectors are created on their own individual layers and by default these layers are switched off to avoid cluttering up your work area. To switch on the layers, display the 'Layer Control' dialog (Ctrl+ L is the shortcut to show / hide this). To show / hide the layer simply click on the check box next to the layer name.

2Rail Sweep Rails - This layer contains two straight line vectors which can be used to sweep a profile along if you are creating a shaped column.

Bounding Box - This layer contains a rectangular vector covering the entire job area. This vector is useful if you are going to machine the complete surface of the cylinder.


Choosing stock material

When setting-up rotary project, software assumes a perfect cylinder with an exact diameter. In practice the stock material may be uneven, or only blank with square profile may be available. In those cases blank needs to be machined into cylinder of desired size, before running toolpaths associated with the actual design.


Another consideration is length of the stock material. Typically, part of the blank will be placed within the chuck. It is also important that during machining, the cutting tool is always in safe distance from both chuck and tailstock. For those reasons, the blank has to be longer than the actual design. When setting-up the machine for cutting, one has to pay extra attention to ensure that origin is set accordingly to avoid the tool running into chuck or tailstock!

If the design was created without those considerations in mind, the blank size can always be adjusted in the Job Setupform.

The picture below presents an example of a rotary project layout. As explained above, the actual blank is longer than job defined in Aspire to allow for the chuck and sufficient gaps. The actual design is shorter than job defined in Aspire, to leave some space for tabs, that can be machined with the profile toolpath prior to removing the finished part from the chuck.

When machining 3D shapes with varying thicknesses like on the example shown below, it is a good idea to place the thicker end of the model on the side closest to the driving motor. This way torsional twisting will mostly affect the stronger end of the machined part and help to avoid bending or breaking of the part during machining.

User Guides | Frequently Asked Questions

User Guides | General Workflow

Cut2D Pro has been developed to allow the production of decorative and artistic dimensional carved parts. As well as drawing and modeling tools, it includes both 2D and 3D machining, along with 3D V-Carving / 3D Engraving to allow a huge variety of jobs to be produced as quickly and easily as possible.

Workflow Logic

  1. Layout 2D Design:
    1. Import Vectors
    2. Draw Vectors
    3. Import Bitmaps
  2. Create 2D, 2.5D or 3D toolpath:
    1. Create or edit vector boundaries for toolpaths
    2. Specify tool details for each strategy
  3. Preview Final Part:
    1. Visualize the part as it will actually look.
    2. Create proof images for customer.
    3. Check estimate for cutting time
  4. Save the CNC Code: Save the final cuto file to send to the CNC machine

Design

Cut2D Pro includes drawing and editing tools that allow designs to be created and modified. Functions for vector creation and editing are very easy to use and multiple design elements can also be drawn or imported, scaled, positioned and interactively edited to make a new design. Text can also be created using any TrueType or OpenType fonts installed on your computer, or the single stroke engraving fonts supplied with the software.

Toolpath

A comprehensive set of 2D, V-Carving, Engraving and 3D toolpath strategies provide you with efficient ways to use your tooling to carve the finished part. This process is usually relatively independent of drawing or modeling (although toolpaths are often created directly from some artwork or 3D composite models). Aspire provides simple interface buttons to toggle screen layout to assist the shift in focus from design to toolpathing.

Output

Finally you can use Cut2D Pro's large selection of post-processors to save toolpaths in precisely the format that your particular CNC machine tool requires.

User Guides | How to Get Started

The first stage in any project is to create a new blank part or import some existing data to work with. At this stage a number of parameters need to be defined relating to the size of the part and its position relative to the datum location on the CNC machine. Later, once the part has been defined and you have started working, you may want to change the size of the material, import additional data and generally manage the project operation. In this section of the manual the initial creation of a part will be covered along with all the icons which appear under the File Operations section of the Drawing Tab.

When you first start the program you will see the Startup Task options on the left hand tab and also a list of your 4 most recently opened Aspire parts (this is a rolling list that will be populated each time you run the software and may initially be empty).


Startup Tasks and Recently Opened Files

When you first start the program you will see the Startup Task options on the left hand tab and also a list of your most recently opened Aspire parts.

The first choice is whether you want to Create a new file or Open an existing one.

The first choice is whether you want to Create a new file or Open an existing one. Creating a new file allows you specify a size and location for a blank work area, set your material thickness and also set the model quality and even the shading color/material. The process to do this will be covered in the next section (Job Setup Form Options).

The second choice, Open an Existing File, will allow you to open a pre-created file from your computer. This may be a file you previously created (*.crv3d or *.crv). Alternatively, it might be a 2D vector layout from another CAD system (*.dxf, *.eps, *.ai and *.pdf). A CRV3D or CRV file will have the necessary information for material size etc. already embedded in it. The 2D formats will import the data at the size and position it was created but will require you to go through the Job Setup form to verify/edit all the parameters for the part.

Video Tutorials

The Tutorial Video Browser will open your default web browser (typically Internet Explorer, Chrome or Firefox - depending on your Windows setup and personal preference). The web browser offers a number of tutorial videos and associated files, presented either by project or feature category to help you to learn about the software. You will initially need internet access to watch or download the videos or files, but, once downloaded, the materials can be used offline.


Online Resources

This section includes direct links to useful websites and web resources - including clipart and projects for you to purchase, download and incorporate into your own designs. These links will also open in your default web browser and you will need internet access to use them.


User Guides | Importing External Models in a Rotary Project

Importing Full-3D models

This section will present the process of importing the Full-3D STL model into rotary project, using a table leg as an example.

A table leg imported from STL file

Overview

There are two basic use cases when importing an external model into the rotary job. The first case involves bringing a model designed for this particular job in another software. Thus the dimensions of the imported piece may already be correct and it can be desired to use them for the size of project. The second use case is when importing a stock model that would have to be scaled to fit on particular machine.

Aspire uses following workflow that covers both of those cases:

  1. Setting-up rotary project
  2. Choosing file for import
  3. Orientating the model in material block
  4. Scaling the model
  5. Finishing the import

Setting up a rotary project

Create a new job using the Job Setup form. It is important to set the job type as rotary to ensure a proper import tool is used in the next step.

If the dimensions of the project are already known, they could be specified directly.

If it is desired to fit the model to a given machine or stock available, set both the diameter and length to maximum. During import the model will be scaled to those limits.

If it is desired to use the imported model size, any size can be specified at this time. During the model import the project can be automatically resized to match the model dimensions.

In this example it was desired to fit the model into a specific stock size with a Diameter of 4 inches and a Length of 12 inches. XY origin was set to centre.

Importing the file and orientating it

To start the importing process, use Import a Component or 3D Model tool from the Modelling tab

Make sure that the Imported model type is set to Full 3D model .

The first step is to position the imported model within the material. This step is necessary as this information is not present in the imported file. When the model was opened, the import tool chose the initial orientation, as can be seen below.

Initial orientation of imported model

To help with orientating the model, the software displays a blue bounding cylinder. This cylinder has the rotation axis aligned with that defined for the material block and thus can be used as a reference. Its size is just big enough to contain the imported model at the current orientation. When the model orientation is changed, this blue cylinder will shrink or grow so it always contains the model. At this stage its exact dimensions are not important, as we are only interested in positioning the model correctly.

The software also highlights the rotation axis in red. This is particularly important when importing bended models. It is currently not possible to represent areas of model that are entirely below or above the rotation axis. This is the case in the example shown here. If the model was imported as is, the distortion would be created as can be seen below. Therefore it is important to position the model in a way such that the rotation axis is contained within the model.

mported model distorted in place where rotation axis was outside the model
The same model imported without distortion

The last guiding element displayed by the software is the red half arrow on the side of the cylinder. This arrow is indicating the position that corresponds to the center of the wrapped dimension in the 2D view. In this example the model is orientated in such a way, that front of the leg would be placed on side of the 2D view, rather than centre. Thus it is better to rotate model so this arrow points to the front of the imported model.

The import tool provides a few ways of adjusting the model orientation. The most basic one is the Initial Orientation. This can be used to roughly align the model with the rotation axis. This can also be combined with the Rotation about Z Axis.In this example the tool chose Left with no rotation. In order to align the front of the leg with the red arrow, one could use the Front and -90 as the Rotation about Z Axis.

Front of the leg aligned with center of the job

Once the initial orientation is decided, further adjustments can be made using the Interactive Rotation. The default option - XYZ View - disables the interactive rotation. That means that the 3D view can be twiddled with a mouse. Selecting other options enables the rotation around the specified axis.

In this example, instead of changing the initial orientation to align the front of the leg with the red arrow, one could select X Model option and rotate the piece manually. When selecting single axis rotation, the 3D view will be adjusted to show that axis pointing towards the screen. If any mistake is made, it is possible to undo rotation using Ctrl+ Z

Notice that whenever the part is rotated, it is always centered in the cylinder. In this example it is not desired, since we need the rotation axis to be contained within the model. In order to move the model in relation to the rotation axis, one can use the Rotation Axis Movement

Similarly to the previously described tool, when Rotation Axis Movement is set to Off, the 3D view can be panned

Correctly positioning the model for importing may require a combination of the Rotation Axis Movement and the Interactive Rotation to achieve desired results with models that bend. It is important to make sure that rotation axis is hidden in order to avoid distortion. However it is also desirable to have the rotation axis being in the center of each segment of the piece to ensure tool has angle close to the optimal during machining. Usually it is also useful to rotate the model in view around the axis after the adjustment, as this allows us to inspect the model from each side without the need to disable the Interactive Rotation before changing the viewing angle.

It is important to understand that Aspire does not support 4-axis machining. That means that while the machined piece can be rotated and tool moves along the rotation axis and in the Z direction, it is not possible to move the tool in the wrapped dimension and thus the tool is always above the rotation axis and cannot be moved to the side.

This limitation is shown below. The first picture presents correct machining of the point. If the tool moves to another location though, the angle will be incorrect and even worse, the tool side will be touching the stock.

3-axis rotary machining, tool correctly positioned
3-axis rotary machining, tool side is touching the stock

Scaling imported model

Once model has been positioned as desired, its size can be taken into account.

By default the tool will assume that imported model is using the same units as the project. If that is not the case, model units can be switched. In this example project was set-up in inches, while imported model was designed in mm. After switching model becomes considerably smaller and a red cylinder, representing current material block is shown, as can be seen below.

Table leg after completing orientation and changing units

At this point it is possible to specify the model size, in terms of diameter and length. This can be done manually by typing desired dimensions, or by fitting to material. If Lock ratio option is selected, the ratio between diameter and length is kept. One can also tick Resize material block option. If it is selected, the material block will be scaled to match current size of the model, after OK is clicked.

If it is desired to use model size as material block size, one can just make sure units are correct, then tick Resize material block option and press OK.

If it is desired for the model to fit material, one could click Scale model to fit material and tick Resize material block.

In this example model was fitted to material. Since in this case length of the piece is limiting factor and lock ratio is maintained, this results in model having considerably smaller diameter than material block. Hence Resize material block option was ticked.

Finishing import

After pressing OK the model will be imported as a component. It is possible to modify it as any other component or add pieces of decorative clipart onto its surface if desired.

It is important to keep in mind the distortion caused by the wrapping process. That means that wrapped toolpaths will match flat toolpaths only at the surface of the blank. The closer to the rotation axis (i.e. deeper) the toolpath is, the more it will be 'compressed'. This fact have a profound implication for 3D toolpaths. Consider the example shown below.

Raster toolpath with constant stepover is compressed in thinner part of model due to distortion

As can be seen if there is substantial difference in diameter in different parts of model, generating one 3D toolpath for whole model will result in wrapped toolpath being overly compressed. Thus it is usually better to create boundaries of regions with significantly different diameter and generate separate toolpaths using correct settings for each diameter.

Importing Flat Models

This section will present a process of importing Flat STL model into rotary project. Flat models are similar to decorative clipart pieces provided with Aspire and are supposed to be placed on the surface of modelled shape.


To start the importing process, use Import a Component or 3D Model tool from the Modelling tab

Make sure that Imported model type is set to Flat model

Initial orientation of imported flat model

Again the first step is to select proper orientation of model. The tool will chose initial orientation and display model in the red material box. This box corresponds to the 'unwrapped' material block and its thickness is equal to half of the specified diameter of the blank.

If model is not oriented correctly, that is, does not lie flat on the bottom of the material box, as can be seen above, orientation have to be adjusted. To do that one can change Initial Orientation option and/or Rotation about Z Axis.

If imported model is not aligned with any of the axes, it may be necessary to use Interactive Rotation.The default option - XYZ View - disables interactive rotation. That means that 3D view can be twiddled with a mouse. Selecting other options enables rotation around specified axis.

Each rotation can be undone by pressing Ctrl+ Z.

Once model is properly orientated, units conversion can be performed. By default the tool will assume that imported model is using the same units as the project. If that is not the case, model units can be switched.

There is also model scaling option included. When Lock ratio option is selected, the ratio between X, Y and Z lengths are kept. Note that once model is imported, it will be added to project as a component. Hence correct placement, rotation and sizing can be performed later, after model is imported.

If the project does not contain any models yet, following message will be displayed:

Typically you could simply click Yes.The more detailed explanation about modelling plane adjustment has been provided in Modelling 3D rotary projects

User Guides | Interface Overview

  1. The Main Menu Bar (the Drop Down Menus) along the top of the screen (File, Edit, Model, Toolpaths, View, Gadgets, Help) provides access to most of the commands available in the software, grouped by function. Click on any of the choices to show a Drop-Down list of the available commands.
  2. The Design Panel is on the left side of the screen. This is where the design tabs can be accessed and the icons within the tabs to create a design.
  3. The Toolpath Tab is on the right side of the screen. The Top section of the toolpaths tab houses all of the icons to create, edit and preview toolpaths. The bottom half shows you toolpaths that you have already created.
  4. The 2D Design window is where the design is drawn, edited and selected ready for machining. Designs can be imported or created directly in the software. This occupies the same area as the 3D View and the display can be toggled between the two using F2 and F3 or the tabs at the top of the window.
  5. The 3D View is where the composite model, toolpaths and the toolpath preview are displayed.
  6. If you wish to see the 2D and 3D views simultaneously, or you wish to switch your focus to the Toolpaths tab at a later stage of your design process, you can use the interface layout buttons (accessible in the 2D View Control section on the Drawing Tab) to toggle between the different preset interface layouts.

Managing the Interface

The tool pages have Auto-Hide / Show behavior which allows them to automatically close when not being used, thus maximizing your working screen area.

The software includes two default layouts, one for designing and one for machining, which can automatically and conveniently set the appropriate auto-hide behavior for each of the tools pages. Toggle layout buttons on each of the tools pages allow you to switch the interface as your focus naturally shifts from the design stage to the toolpathing stage of your project.


Accessing Auto-hidden tabs

If a tools page is auto-hidden (because it is currently unpinned, see pinning and unpinning tools pages, below), then it will only appear as a tab at the side of your screen. Move your mouse over these tabs to show the page temporarily. Once you have selected a tool from the page, it will automatically hide itself again.

Pinning and unpinning tools pages

The auto-hide behavior of each tools page can be controlled using the push-pin icons at the top right of the title area of each page.

Default layout for Design and Toolpaths

Aspire has two default tool page layouts that are designed to assist the usual workflow of design, followed by toolpath creation.

In all three of the tools tabs there are 'Switch Layout' buttons. In the Drawing and Modeling tabs, these buttons will shift the interface's focus to toolpath tasks by 'pinning-out' the Toolpaths tools tab, and 'unpinning' the Drawing and Modeling tools tabs. In the toolpaths tab, the button reverses the layout - unpinning the toolpaths page, and pinning-out the Drawing and Modeling pages.You can toggle between these two modes using the F11 and F12 shortcut keys.

User Guides | Modelling 3D Rotary Projects

Elaborating 2D designs with 3D clipart pieces

[object Object]
Fluted column with added 3D clipart

This section will present how to add 3D clipart to basic fluted column presented in Simple rotary modelling using 2D toolpaths.

A simple way to start with 3D rotary models is to use add pieces of decorative clipart that is provided with Aspire. This process is very similar to adding clipart to single- or double- sided project, however there are some additional considerations that are specific to wrapped rotary machining.

To start, switch to the Clipart tab. Then choose a piece of clipart and drag and drop it into the workspace. Aspire will show following message:

To understand this message, we need to consider the flat view of our model, after importing the clipart. Flat view can be accessed by clicking Auto Wrapping button.

As can be seen, the model contains only the selected decorative piece on the flat plane. Although the column is obviously a cylindrical solid, so far we only used 2D toolpaths to carve details on the surface of cylinder. So the fact that machined piece is a cylindrical solid, derives only from fact that the blank is a cylindrical solid itself. Aspire allows the 3D model to also describe a solid body.

In this example the intent is to only place a decorative piece on the surface, rather than define body of the column. Aspire can see that we did not model a body and we are placing a piece of clipart, that is likely to be placed at the surface. By responding 'Yes' to the message we can confirm that it is our intent to use the component to decorate a surface.

Note

The above message is only displayed when the 3D model is empty. Regardless of user choice, this message will not be displayed again for this project.

More clipart can be placed as desired. Then the 3D view can be inspected. Once design is finished it is time to create toolpaths. In order to create 3D roughing toolpath, use 3D Rough Toolpath. Then create 3D finishing toolpath, using 3D Finish Toolpath. Select settings that are most appropriate for given application, while remembering which axis is rotating. The choice of axis may be particularly important if rotation axis speed is slower than linear axis.

In this example the decorative clipart that was added was not recessed. That means that after 3D machining the flat areas around clipart will be recessed due to clipart 'standing out' of the flat surface. Therefore existing 2D toolpaths needs to be projected. This can be accomplished by selecting Project toolpath onto 3D model option and recalculating the toolpaths.

Making a tapered column

Simulation result for tapered column model

This section will explain how to make a tapered column by modifying the basic design from previous section.

So far only the surface details were modelled. In order to make a tapered shape, we need to model 'body' of the shape in addition to surface details. For that purpose, zero plane component can be used. It is added automatically for rotary jobs.

Double-click zero plane component to open Component Properties. Enter 0.8 in the Base Height box. Select Tilt option. Click Set button in Tilt section, then switch to 2D view and then click in the middle left and then in the middle right. Set angle to 3 degrees.

Since the modelling plane was adjusted for placing component on the surface, it needs to be adjusted again, so the component body is not 'inflated'. To do that open Material Setup form. Adjust modelling plane by moving slider down, until Gap Inside Model is 0.

Modelling plane position when designing the 'body' of a shape

After modelling a tapered shape, the 3D model of column will have a desired shape. However clipart pieces in the narrower parts have been distorted, as can be seen below. To fix that, one need to stretch the components in the wrapped dimension, to compensate for distortion.

Tapered column with distorted clipart
Tapered column with clipart stretched to overcome distortion

The distortion that has been demonstrated above, applies also to toolpaths. That means that wrapped toolpaths will match flat toolpaths only at the surface of the blank. The closer to the rotation axis (i.e. deeper) the toolpath is, the more it will be 'compressed'. This fact have a profound implication for 3D toolpaths. Consider the example shown below.

Raster toolpath with constant stepover is compressed in thinner part of model due to distortion

As can be seen if there is substantial difference in diameter in different parts of model, generating one 3D toolpath for whole model will result in wrapped toolpath being overly compressed. Thus it is usually better to create boundaries of regions with significantly different diameter and generate separate toolpaths using correct settings for each diameter.

Modelling turned shapes

A chess pawn

This section will present a basic technique for creating turned shapes.

Modelling turned shapes is quite easy. It requires a vector representing a profile of the desired shape and a Two Rail Sweep tool.

To start, create a new rotary job. Then either draw a profile using available drawing tools or import profile vector. This example used a chess pawn profile, as can be seen below.

A chess pawn profile vector

Open the Two Rail Sweep tool. When the rotary job is created, the software inserts a special layer called '2Rail Sweep Rails'. It contains two blue lines on the sides of the job, that are perpendicular to the rotation axis.

Select both of those rails and click Use Selection button. The rails will be highlighted. Then select the profile vector and click apply. Inspect the 3D view to verify the results.

Modelling cross section

A Hexagonal Column

This section will explain how to model desired shape using Vector Unwrapper.

Vector Unwrapper is useful when rather than modelling a profile along the rotation axis, it is more intuitive to specify desired cross section. The tool transforms a vector, representing a cross section, into a profile vector that can be subsequently used with Two Rail Sweep tool.

Suppose we would like to create a hexagonal-shaped column. Let's start by creating a new rotary job. In this example job has a diameter of 6 inches and is 20 inches long. X axis is the rotation axis and Z origin has been placed on the cylinder axis.

We need to create a hexagon using Draw Polygon tool. This vector will serve as a cross section and can be placed anywhere in the 2D view. In this example the material block diameter is 6 inches, so the radius of the shape cannot exceed 3 inches.

When the shape is created, select it and open Vector Unwrapper. The tool will display a cross hair in place where the rotation axis is crossing the profile and a circle with the diameter of the material block. This will help you determine whether the shape with such cross profile will fit in current material block.

2D view with Vector Unwrapper tool active

In this example, Use Center of contour option was used. That means that rotation axis will be placed in the centre of vector's bounding box. One can also tick Simplify unwrapped vectors option to fit bezier curves, instead of using series of very short line segments. After apply is pressed, the unwrapped version of the selected cross section will be created, as have been shown below.

Results of 'unwrapping' the hexagonal cross section

This example shows the unwrapped vector for a cylinder rotating around the X axis. If your rotary axis is aligned along Y the unwrapped vector will be horizontal. It is worth noting that unwrapped profile have 'legs' on each end. Those are needed to ensure that correct height will be used in the next step.

The tool automatically creates layer called 'Unwrapped Vectors Drive Rails' on which it places two blue line vectors on job sides, parallel to the rotation axis. In order to extrude the profile, open the Two Rail Sweep tool. Then select top and then bottom rail (left and right when Y axis is rotation axis) and confirm selection by clicking Use Selection button. Rails will become highlighted. Now click on unwrapped vector and press apply. The 3D view will show a hexagonal column, that can be seen at the beginning of this section.

Modeling Plane

The desired cross-section will only be achieved if modelling plane is positioned in cylinder centre. That means that Gap Inside Model is reported as 0 in Material Setup form. Otherwise the resulting model will have incorrect diameter and the cross section will become rounded.

Vector unwrapper is not restricted to simple shapes. In principle it is always possible to use convex shapes and certain concave shapes. The example below shows a heart profile unwrapped.

Heart-shaped vector and its unwrapped version
Extruded heart shape

If cross section in question is concave, one could imagine straight line starting in the center of the shape and touching a point on the boundary. If the second points keeps travelling along the boundary and each line is not crossing another point on the boundary, then it is possible to use this cross section. If the line does cross more than one point on the boundary, this part of the cross section will not be represented correctly.

All the examples so far used a single cross section. However it is also possible to use multiple cross sections.

Let's take another cross section and open Vector Unwrapper. Then drag the rotation axis handle a bit down from the center. If snapping is enabled, it can be used to help position the rotation center, as can be seen below.

Rotation center is being dragged. Snapping feature is used to position handle accurately

Once we have another unwrapped cross section, it is possible to use both during Two Rail Sweep. For example unwrapped heart profile can be placed twice on the left and twice on the right. The second unwrapped profile can be placed twice in the middle. Such arrangement may result in shape morphing, as can be seen below.

Two different cross sections used in Two Rail Sweep
Morphed shape

User Guides | Post Processor Editing

What does the Post Processor Do?

The post processor is the section of the program that converts the XYZ coordinates for the tool moves into a format that is suitable for a particular router or machine tool. This document details how to create and edit the configuration files that customize the output from the program to suit a particular machine control.

Below are sections of a typical program that has been post processed into both G-Code and HPGL

G-Code Output

T1 M6

G17

G0 Z4.5000

G0 X0.0000 Y0.0000 S12000 M3

G0 X2.4567 Y7.8342 Z0.2500

G1 Z-0.0500 F5.0

G3 X3.3784 Y8.7559 I0.0000 J0.9218 F66.0

G3 X2.4567 Y9.6777 I-0.9218 J0.0000

G3 X1.5349 Y8.7559 I0.0000 J-0.9218

HPGL Output

IN;PA;

PU2496,7960;

PD2496,7960;

AA2496,8896,90.000

AA2496,8896,90.000

AA2496,8896,90.000

AA2496,8896,90.000

PU2496,7960;

PU2496,6096;

Machine controller manufacturers will often customize the file format required for programs to run on a particular machine in order to optimize the control to suit the individual characteristics of that machine.

The Vectric post processor uses simple text based configuration files, to enable the user to tailor a configuration file, should they wish to do so.

Post Processor Sections

Vectric post processors are broken down into sections to aid clarity, try to write your post processors in a similar style to aid debugging.

File Comments

A section where you can describe the post processor and record any changes to the post processor, each line is a comment and starts with a ‘+’ character or a ‘|’ character.

+ History

+ Who When What

+ ======== ========== ===========================

+ Tony 14/07/2006 Written

+ Mark 26/08/2008 Combined ATC commands, stop spindle on TC

+================================================

Global File Statements

Statements are items that are either used only once, or have static values throughout the file. Write statement names in upper case letters for clarity.

Statement

Result

POST_NAME="Text Output Arcs(mm)(*.txt)

The name that will appear in the post processor list

FILE_EXTENSION="txt"

The file extension that the file will be given

UNITS="MM"

The units that the file outputs (INCHES or MM)

PRINT_DIRECT="YES"

The machine tool manufacturer has supplied a driver (usually a printer driver) thatn can directly accept the NC file output (For example see Generic HPCL_Arcs.pp)

RAPID_PLUNGE_TO_STARTZ="YES"

Indicates that plunge moves to Plunge (Z2) height (that is set on the material setup form) are rapid moves

DIRECT_OUTPUT="Display Name|Manufacturers.Document"

The control software uses a document interface that can directly accept the NC file output.

ROTARY_WRAP_Y=A

The moves in the Y axis are to be wrapped around a cylinder of the specified diameter. The "Y" values will be output as "A"

ROTARY_WRAP_X=B

The moves in the X axis are to be wrapped around a cylinder of the specified diameter. The "X" values will be output as "B"

SPINDLE_SPEED_RANGE = 1 15 4500 15000

Spindle speed for this machine is output as a range of integer numbers between 1 and 15 representing the actual speed in RPM of the spindle, (between 4500 and 15000 RPM in the quoted example). For an example, see the file: Roland_MDX-40_mm.pp

SUBSTITUTE = "O1 S1 O2 S2 On Sn"

This command allows you to substitute a character output within the variables (such as [TOOL_NAME]) and substitute that character, with another. This feature can be useful for those cases where particular characters cause errors on an NC control.

The characters are entered in pairs, Original - Subsititued.

For example MACH 3 control software uses parentheses as comment delimiters, and does not allow nested comments. Most tools within the Vectric Tool Database have parentheses within the “Name” section; if these names are output, this would cause an error within Mach3. The command SUBSTITUTE = "({)} " would convert the () characters to {} characters, and avoid this error. For an example, see the file: Mach2_3_ATC_Arcs_inch.pp

Tape Splitting Support

A section that describes how a long toolpath output will be split:

TAPE_SPLITTING=MAX_NUM_LINES LINE_TOL "FILENAME_FORMAT" START_INDEX INDEX_ON_FIRST_FILE

For example a command of:

TAPLE_SPLITTING=1000 100 "%s_%s.tap" 1 "YES"

would lead to...

Output will be split into multiple files of a maximum of 1000 lines (+ however many lines in there are within the footer section of the post processor), if a retract move exists after line 900 (1000 – 100), the file will be split at that move. If the file was called "toolpath" the split files would be named toolpath_1.tap, toolpath_2.tap etc. The first toolpath output will be "toolpath_ 1.tap" there will be no file named "toolpath" without an index number, (as INDEX_ON_FIRST_FILE= YES is used), unless the file was less than 1000 lines long, in which case the file would not be split.

Note

Some controllers that require NC files to be split, also have limitations on the number of characters within a filename. For example they may require the file to be named with the MSDOS style 8.3 filename format. This should be considered when naming the output file.

Line Terminating Characters

LINE_ENDING="[13][12]"

Decimal values of the characters appended to each separate line of the post processed file. (Will usually be [13][10]) (Carriage return, line feed) for any controller that can read a windows or MSDOS format text file.

Block Numbering

If you wish to add line numbers to the output file, the current line number is added with the variable [N]. The behaviour of this line number variable is controlled by the following variables:

Statement

Result

LINE_NUMBER=0

Value at which the line numbering should start

LINE_NUMBER_INCREMENT=10

Incremental value between line numbers

LINE_NUMBER_MAXIMUM=99999

The maximum line number to output, before cycling to the LINE_NUMBER_START value again.

Important - Some controllers have a limit to the number of lines that can be displayed on the control

Variables