Cut2D Desktop User Manual

Version 9

☆ What's New ☆ Disclaimer Introduction Overview of the Interface Managing the Interface 2D Design and Management Two-Sided Machining Frequently Asked Questions FAQ Glossary

How to Get Started Job Setup Calculation Edit Boxes Document Variables View Controls Main Menu Right Mouse Click menus Rulers, Guide Lines and Snapping Shortcut Keys

Click on the region of the interface you are interested in:

Disclaimer

All CNC machines (routing, engraving, and milling) are potentially dangerous and because Vectric Ltd. has no control over how the software described in this manual might be used, Vectric Ltd. or any associated Resellers cannot accept responsibility for any loss or damage to the work piece, machine or any individual, howsoever caused by misusing the software. Extreme care should always be taken and the output from the software thoroughly checked before sending it to a CNC machine.

The information in this manual may be subject to change without any prior notice. The software described in this manual is supplied under the terms and conditions of the software license agreement and may only be used in accordance with the terms of this agreement.

Vectric Ltd.
Web: www.vectric.com
Email: info@vectric.com
Phone: +44 (0) 1527 850 323
Fax: +44 (0) 1527 850 323

Introduction

This manual is designed to provide a comprehensive description of all the functions, tools, menus and icons available within the Cut2D Desktop software package.

Access this document from Cut2D Desktop's Help Menu ► Help Contents or from the Cut2D Desktop folder in the program section of your Windows Start menu.

At the bottom of the page you will see an area with View All Help. This will download all the Help Documentation as a single web page which is useful for searching or if you need to create a paper copy of the documentation.

User Guides, tutorial and training

Please note that this document is a Reference Manual. If you require more guidance, or are still learning how to use Cut2D Desktop, please ensure that you view the Getting Started Video Tutorials in the Cut2D Desktop Video Tutorial Browser when starting the software.

Cut2D Desktop also includes an extensive selection of video tutorials, which are accessible from the Tutorial Video Browser link when application first starts. These tutorials cover every aspect of Cut2D Desktop's functionality and range in complexity from a beginner's overview, to advanced features and principles. They are intended to be extremely accessible by level of experience or topic and use real-world examples throughout. Videos can be watched online, or installed locally.

We welcome any comments on this manual or the other training material, please email support@vectric.com with your feedback.

Overview of the Interface

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 Drawing and Layers tab 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 Cut2D Desktop. 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 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 Drawing, Layers and Toolpath tool pages have Auto-Hide / Show behavior which allows them to automatically close when not being used, thus maximizing your working screen area.

Cut2D Desktop 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.

			Pinned Open (auto-hide disabled)
			Un-pinned (auto-hide enabled)

Default layout for Design and Toolpaths

Cut2D Desktop has two default tool page layouts that are designed to assist the usual workflow of design, followed by toolpath creation.

View Controls

Your project is represented using 2D and 3D workspaces, each viewed via independent windows called 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.

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

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
	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
	Side View (Along X)	Shows the side view of the model in the 3D View looking along the X axis
	Side View (Along Y)	Shows the side view of the model in the 3D View looking along the Y axis

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 Cut2D Desktop 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 Cut2D Desktop 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 in Aspire (*.crv3d), or a VCarve Pro job (*.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.

Two-Sided Machining

Cut2D Desktop has the ability to create a project where your design requires you to cut both sides of your material. Typically you will cut the top surface of your material, then manually turn the material block over on your machine, whilst maintaining a common registration position, and cut the bottom surface using a second set of toolpaths. By specifying a two-sided project using the Job Setup form and indicating how you intend to flip the material over on your machine, you can allow the registration and organisation of the geometry, toolpaths and previews relating to each side of the design to be managed by the software. During the design process you can then switch between the top and bottom surface of your design, create toolpaths for each side and view a preview of the material - including after it has been cut from both directions. Once you are happy with the result you can then save the toolpaths relating to each side independently.

Two-Sided Job Setup

In the Job Setup dialog, you can pick whether you want to create a single-sided or a double-sided job. You can change this setting later if you wish.

The initial Z-Zero Position you will be using for the toolpaths relating to each side is set from the Job Setup dialog. You can choose to Z-Zero from the same material surface for both sides, the machine bed for both sides or you can opt to Z-Zero from each side indepenendently. Your choice depends on the nature of your design. Typically, if you are only intending to carve into the surface on each side then you will Z-Zero each independently after you have physically positioned the material on your machine. If your design involves cutting through the material and the Z depths for each side must coincide precisely, however, then you will usually wish to use a common Z position for both sides. You can change the Z-Zero settings for each side subsequently using the Material Setup form.

The X Y Datum Position applies to both sides of the material.

In order to correctly manage the alignment of the geometry relating to each side, it is important that the software knows whether material will be flipped vertically or horizontally during the physical machining process. Flip Direction Between Sides determines the automatic transformation of the drawings, models or toolpaths associated with each side. If the material block will be flipped horizontally then the software will automatically mirror your data to mimick the relative positions each side.

When you create or open a two-sided project, Cut2D Desktop will display two new icons in the 2D View Toolbar. The first icon indicates which flip direction option has been specified for this project. It will ininitially be set to display the Top Side of your design. Any drawing or toolpath creation will be associated with the Top Side and this is known as the active side. To work on the other side of your design you will first need to make the Bottom Side active. Click on the Toggle Side button in the View Toolbar to switch the active side between top and bottom. Alternatively, you can use the number key shortcuts: 1 will make Top Side active and pressing 2 will make the Bottom Side active.

Two-Sided Toolpath Management

When toolpaths are created in a two-sided job they are automatically associated with the active side from which they were created. This helps you to keep track of which side of your job each toolpath is for. The toolpath list will only display the toolpaths for the current active side and this is indicated in the heading, which will read Toolpaths (Top) or Toolpaths (Bottom) accordingly. Changing the active side (using 1 or 2, for example) will cause the toolpaths list to also swap the displayed set of toolpaths.

Two-Sided Toolpath Previewing

The Preview Toolpaths form now includes a Preview All Sides button. This will simulate toolpaths cutting both sides of your job (regardless of the currently active side) so that you can see the combined result of your toolpaths in a single, solid, 3D representation of the final job.

Two-Sided Toolpath Saving

Saving your toolpaths from a two-sided job is done independently for each side. Save the toolpaths for the currently active side, then make the other side active (using 1 or 2) and save out the toolpaths for the other side.

The View Toolbar

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

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.

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.

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

2D Design and Management

The 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 Cut2D Desktop 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 Cut2D Desktop, 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. Cut2D Desktop 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. Cut2D Desktop 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, Cut2D Desktop 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.

Vectors

Vectors have two very important uses:

1. To describe the shape/boundary/direction of a toolpath
2. To control 3D shapes created using the icons under the Modeling Tools

As they are such an important part of two of the fundamental areas of the software there are a lot of tools to create, edit and manage them. In this section all these tools and vectors options will be briefly described. For practical examples of these tools you should review the tutorial videos.

Vector Import

Decorative vector designs and shapes will often be imported from another drawing package such as Corel Draw, AutoCAD etc. rather than being completely drawn in Cut2D Desktop. The Vector Import icon is located in the File Operations area of the Drawing Tab. Once a vector has been imported then the imported vector shape(s) can be modified, moved, scaled, rotated, mirrored or deleted the same as vectors created within the software.

The following Vector file formats can imported

While every endeavor is made to keep up with other software companies' changes in their file format it is possible that files in the above formats may not always be readable in Cut2D Desktop. In that case going back to the original design systems and saving the file in an earlier version may enable it to be loaded into Cut2D Desktop. In addition Cut2D Desktop may not support the import of special entities such as dimensions, hatching, text, numbers etc. from some vector file types. It may be possible to adjust the formatting for these objects in their original design program. This is often done using a command called Convert to Curves. This will change this type of data to regular vectors that can then be exported in a compatible format for import.

Program Options

1. Window Layout
2. 3D View Settings
3. Toolpath Settings
4. General Settings

Window Layout

Toolpath Settings

General Settings

Rulers, Guide Lines and Snapping

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↓

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 Apply. 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 Create New Guide.

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 Menu. Guide Lines can be Deleted by selecting View Menu ► Guide Lines ► Delete All Guides from the Main Menu. Individual Guide Lines can be deleted by clicking and dragging them out of the 2D View Window.

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 Menu or by pressing F4.

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.

Snap to Nodes, mid-points, centers

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.

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

Cursor	Type	Color	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	(No line)	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

Object Centre

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

Horizontal

Tangents

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

Tangent

Perpendicular to Tangents

These snap lines will be 90° from the tangent snap line, and they both

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.

Connecting Lines

Span Geometry

Span geometry

Angular Constraints

Angular Constraints eg. 30° (Angle step 15°)

Job Edges & Centre

If you have the job snapping enabled, you could snap to the horizontal and vertical middle lines. This, also, includes the lines extending from the job's edges.

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.

Document Variables

Document Variables provide a mechanism for defining values that can be used in Cut2D Desktop's Document Variables. They can either be created in the Document Variables dialog (right) 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

Right-click an edit-box to insert a new or existing Document Variable:

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 fo 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.

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 Desktop's stored values can be accessed by using certain letters (which are not case-sensitive): When used, Cut2D Desktop substitutes the character with the appropriate value in the calculation.

The Drawing Tab

Cut2D Desktop includes drawing and editing tools that allow designs to be created and modified, which can ultimately be used directly for toolpath creation.

Commands 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.

File Operations

Click on an icon to learn more about it:

File Operations

New, Open and Save

Create a New File	This option opens the Job Setup form (below), which is used to create a new blank job of the width (X), height (Y), and thickness (Z) required. 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.
Open a File	This option opens the File Open dialog window, allowing Cut2D Desktop files (CRV) and importable 2D vector files to be selected and opened.
Save a File	This option opens the File Save As dialog window and allows the job to be saved as a Cut2D Desktop file. Navigate to the required folder, enter a suitable name for the job and click the Save button.
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 Cut2D Desktop. 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 main menu bar. Any Toolpath data saved as .PVC or .V3D files can be imported and will be visible in the Toolpath List.
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.

File Types

SketchUp Files

SketchUp files with a .SKP extension (see www.sketchup.com) can be imported as 2D data suitable for machining into a Cut2D Desktop 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.

When the SketchUp model is selected from the File Import dialog, the following dialog will be displayed.

Although this initially looks complex, the dialog is divided into four logical sections which will be describe below.

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.

We will describe the 'Three Views - Front, Top, Side' option first as it is the simplest.

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.

Exploded Flat Layout

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

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

Part Orientation

This section controls what Cut2D Desktop 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 Desktop can be used to layout the parts with more control and across multiple sheets.

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 Desktop offers the option to refit circles and arcs to imported data.

Options Checked ✓

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 Desktop 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 Desktop. The screenshot below shows the result of only importing data on the 'Door' layer from the example.

As long as the 'Group imported parts' option is selected, these parts can then be easily nested ready for machining as shown in the image below (the 'Group imported parts' option is explained later in this section).

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 Desktop 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 Desktop. 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 Desktop 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 Desktop 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 Desktop 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 Desktop 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.

Cut, Copy and Paste

The Cut, Copy and Paste functions in Cut2D Desktop can be used on Vectors or Bitmaps.

Cut	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.
Copy	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.
Paste	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 Desktop parts.
Undo	Clicking this option steps backwards through the design changes made by the user.
Redo	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.

Job Setup

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.

Job Type

Select Single Sided if your design only requires the material to be cut from one side. This is the simplest type of job to design and machine.

If your design requires you to cut both sides of your material then Cut2D Desktop also allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file. Select Double Sided if you need this additional functionality.

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).

Height

The material length along the Y axis

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 position.

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 OK.

The Create Vectors Tool Group

Click on an icon to learn more about it:

Create Vectors
					Closed Shapes
					Open Shapes
					Creating Text
					Trace Bitmap     Dimensions

Drawing Shapes

Each tool gives you the option of dynamically drawing with the mouse in the 2D View, or entering precise data using the form. When you click on a shape tool icon its associated form will open on the Drawing tab. Here you can see the precise dimensions of the shape you are working on, which you can edit directly, as well as other options specific to the type of shape you are editing.

If you click on a shape drawing tool when nothing is selected in the 2D View, you will be able to create new shapes using the Create button. If you select a previously created shape, you will be able to modify its properties using the same form and update the shape using the Apply button.

Creating Text

There are a number of tools dedicated to the creation and editing of text. These can be found on the Drawing tab, below the shape creation tools.

Cut2D Desktop can make use of any TrueType font already installed on your computer, as well as Vectric's own single-line fonts designed specifically for CNC machining.

Use the Draw Text, or Draw Auto Text, to create text within your design. The Text selection tool then allows you to dynamically alter the text positioning, spacing or even to bend your text into an arc. For even more flexibility, use the Text on Curve tool to place your text along any vector curve or line that you have drawn. The Convert Text to Curves tool allows you to then use Node Editing to fine tune the vectors of the text to any shape required.

The text tools are accessed using the following icons:

Create Text

Auto Layout Text

Text Selection

Convert Text to Curves

Text on a Curve

Trace Bitmap

Trace Bitmap tool allows you to automatically trace imported bitmaps using a variety of options within the tool to control the vectors that are created.

Dimensions

The dimensions tool allows you to add a variety of dimensioning annotations to your vector 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.

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).

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:

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 Create 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 Apply 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 Close on the form
• Press the Esc key
• Click the Right mouse button in the 2D View.

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.

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.

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 ValueEnter or Diameter,Enter to create an ellipse with the specified dimensions.

Example

Specifying Further Properties

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

Examples

Exact Size

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

Edit

• 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 Apply to update the ellipse.

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

Close the form

To finish drawing with the tool, you can:

• Click Close on the form
• Press the Esc key
• Click with the Right-mouse button in the 2D View

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 - Cursor

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.

As the cursor is dragged across the screen so the XY size 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, 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 ValueEnter or Side Length,Enter to create a rectangle with the specified width and height.

Example

Specifying Further Properties

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

Examples

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.

Edit

• 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.

Close the form

To finish drawing with the tool, you can:

• Click Close on the form
• Press the Esc key
• Click the Right mouse button in the 2D View.

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 - Cursor

• 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.

As the cursor is dragged across the screen so the 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 values will be used to set the radius of your polygon. While you are dragging out the polygon, type Radius ValueEnter to create a polygon with the precisely specified radius.

Example

Specifying Further Properties

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

Examples

Exact Size

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

• Click Apply to update the circle.

Edit

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

The selected circle is displayed as a dotted magenta line.

• Edit the Number of Sides and Radius.
• Click Apply to update the circle.

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

Close the form

To finish drawing with the tool, you can:

• Click Close on the form
• Press the Esc key
• Click the Right mouse button in the 2D View.

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 - cursor

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.

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 ValueEnter to create a star with the precisely specified outer radius.

Example

Specifying Further Properties

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

Examples

Exact Size

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

• Click Create to update the star.

Edit

• 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.

Close the form

To finish drawing with the tool, you can:

• Click Close on the form
• Press the Esc key
• Click the Right mouse button in the 2D View.

Draw Polyline

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 Spacebar to complete this polyline but keep the form open and begin drawing another polyline.

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.

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.

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 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 ValueEnter 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 ValueEnter to place the next point precisely at specified X and Y position.

Example

Specifying Further Properties

By using specific letter keys after your values, you can also specify the line segment in terms of angle and length.

Examples

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

Create 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.

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 Create 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 Apply to update the selected arc with the new values.

Draw Curve

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

• 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.

Create 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.

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

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

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

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

Medium 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.

Applications

The vectors created by this function have many applications but a key one is to combine them with either a Profile Toolpath or where available the Texture Toolpath to create decorative panels and background textures, a small selection of the possible results you can derive from this combination are shown in the images below.

Ball Nose Tool - Wave Pattern

V-Bit Tool - Swirl Pattern

Ball Nose Tool - Grain Pattern

Create Text

This form allows text to be created at any height using the units the model is being designed in (Inch or MM).

Vertical Fonts

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

Vertical Text

Engraving Fonts

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

Options

The Larger Edit... button opens a larger text entry window that makes it easier to enter text that needs to run on longer line lengths. Clicking OK accepts any text entered into the window and Cancel will throw away any changes.

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 and click Apply, or click in the 2D View with the mouse cursor to set the position values interactively. Clicking in the 2D View will begin a new block of text, set to the new Anchor point.

Edit Text

To edit text properties or content of previously created text:
If the Create Text form is open, hold the Shift key down and 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.

Click the Apply button to update the changes in the 2D View. Click the Cancel button to finish or cancel the editing and close the form.

Draw Text Within A Box

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.

When the Text form is open, the Dimensions for the Width and Height of the selected vectors or job dimensions are shown, and these are used to constrain the font size of the text.

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
• Click Apply

Vertical Fonts

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

Vertical Text

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:

Options

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

Clicking OK accepts any text entered into the window and Cancel will throw away any changes.

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.

None

Normal

Wide

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

Stretch Line Space 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

Stretch Spaces between words

Stretch Kerning (space between letters)

Stretch Character size

Edit Text

To edit text properties or content of previously created text:
If the Create Text form is open, hold the Shift key down and 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.

Click the Apply button to update the changes in the 2D View. Click the Cancel button to finish or cancel the editing and close the form.

Text Selection

Interactive Letter kerning and Line Spacing

Select the cursor and click to select the Text to be edited. The text will be displayed as lines with 2 Green handles in the middle:

Letter Kerning

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

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:

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 Arcing

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

Bend Text Upwards

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 using the green boxes.

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

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.

Clicking and dragging the Blue boxes moves the text vertically and changes the radius onto which the text is mapped:

Convert text to Curves

In most cases all Text created in Cut2D Desktop can be VCarved, Engraved, Pocketed and Profile machined or used with the 3D modeling functions. Some fonts do occasionally include loops and problems that need fixing using the Node Editing tools before it can be utilized for other functions. This text first has to be converted to Curves, creating lines, arcs and Bezier spans that can be interactively edited to fix the problem areas.

Script style fonts that are based on overlapping characters can be VCarved or Engraved without having to first convert the characters to curves.

If the individual characters contain overlapping vectors or loops these will need fixing manually using the Node editing tools.

When Profile Machining with Tabs is required the text must first be converted to curves. Opening the Tab form on the Profile machining form will show a message stating that the text must first be converted to curves and clicking the Yes button will automatically make the conversion.

Text can be converted to curves at any time by selecting the icon or clicking the Right mouse button and selecting Convert Text to Curves.

Text on 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.

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.

Text Position

The position of text relative to the curve is calculated using the height of the largest letter in the selected text string.

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.

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

Align to Curve

Keep Vertical

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.

Images can be traced either in color or black and white mode and the basic process is described below:

If the image is black and white already, the process can be considerably simplified by selecting the Black/White option.

For color images you can also reduce the number of colors you need to work with by using the slider to further simplify the trace selection process.

Check ✓ the boxes next to each color swatch to link colors to the Trace Color. These are the colors that will be included in the area to trace.

Adjust the fitting parameters for the resulting vector and use the Preview button to trace.

Click the Apply button when you are happy with the preview.

After vector fitting you will often need to adjust the vectors so be sure to watch the video tutorials on vector editing available for the software.

Working with 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.

Working with 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 Preview button automatically creates vector boundaries either around the selected Trace Color or the grayscale.

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

Tight

Loose

Loose will create smooth curves that may not follow corners very precisely, but will create smooth free-flowing vectorboundaries, with few nodes.

Tight

Tight inserts nodes to ensure the vector accurately follows the color boundary, to create sharp detail.

When using the Trace Color option it's sometimes useful to link a region of color's together, fit vectors and then link a new region or color's together, un-check the replace existing vectors option and fit another set of vector boundaries.

Noise Filter

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

For example, if an image contains single or very small clusters of pixels that aren't needed for machining a design. Then using the noise filter slider set at 4 pixels will ignore 2 x 2 or smaller pixel clusters.

Bitmap Fading

The Bitmap Fading slider controls the shading of the image in the 2D View. This is useful to see the trace vectors more clearly over high-contrast images.

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 Preview button again to get an updated result.

Apply

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

Close

Closes the Trace Bitmap form.

Dimensions

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

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

1. Select the dimension type you wish to need: length; height; width; angle or the radius or diameter of an arc.
2. 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.
3. Click where you need the arrow-tips to be.
4. Click to set the location of the dimension-line.
5. Click to set where the annotation text will appear.

• While dragging out a new dimension, a preview rectangle indicating the text size and position will be drawn.
• If you select a dimension before opening the Dimensions Form, the font properties can now be edited. Changing dimension-type or clicking a point on the screen while the form is open will start the creation of a new dimension.
• To edit an existing dimension while the form is open, hold down a Shift key while selecting it - there is a note on the form to remind you of this.
• When creating Dimensions, the mouse snaps onto vectors, guide lines and the four corners / mid-points around the edge of the job setup area unless a Shift key is held down while dragging.
  
  Arc Dimensions snapped to a guide line

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).

The text in the following example was first converted to vectors using the Convert Text to Curves command, then those vectors were converted to arcs using the Fit Curves to Vectors command:

Further Angle Dimension Examples:

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.

The base of extension lines and the tips of arrows are snap-points allowing you to keep neighbouring linear dimension lines, lined up, for example.

Transform Objects

Click on an icon to learn more about it:

File Operations

The Transform Objects section contains all the icons which relate to commands for moving, sizing and manipulating objects.

Quick Keys

This reduces the time to create accurate geometry by allowing typed values while creating geometry. This is supported for creation of circles, ellipses, rectangles, polygons, stars, polylines and when in editing nodes or transforming vectors.

For example, while dragging to create a circle, typing 3R will create a circle with a radius of 3.

Inputting a Value

Input mechanism is as follows:

1. Input the value first, and Enter to execute the default action (if applicable)
2. Input the value first, and then a letter indicating the type of action required.
3. Input 2 values separated by a comma, and Enter to execute a specified action (usually width and height or X and Y).

1. Some actions require several input values.
2. In that case, it will be valuelettervalueletter
3. The action will be performed automatically once all letters required for that action have been entered.

You can enter a value and press Enter which will perform the default action.

The input times out after 5 seconds, if nothing was entered.

The value could be a simple expression, similar to that used from some of our text fields.

A full list of shortcuts can be found on the Shortcuts page

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

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.

Move Interactive

The default mode is to enable selected objects to be moved interactively by clicking and dragging with the cursor.

Holding down the Alt key when dragging objects around will constrain the movement to either the X or Y axes.

Pressing Esc or clicking Close will close the form.

Quick Keys

For moving objects with a specific amount without having to go into the form, the Quick Keys can be used while dragging the object. Simply, activate interactive movement by clicking twice on the object, and then drag it and start typing the value as per the shortcut keys table. Then, either press Enter or the letter required to perform your action.

See Quick Keys shortcut table for a list of available actions.

Smart Snapping

To constrain the movement of the object in the X or Y axis, start dragging the object along that axis and a snap line will appear that represent that axis.

This can be used in combination with the Quick Keys, mentioned above, to move the object by a set amount in a specific direction.

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.

Size Interactive

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

1. Select the vectors
2. Click a second time to activate the interactive options - handles on the selection box
3. Click and drag on the white handles

The keyboard shortcut T opens the Scale form in interactive mode.

Interactive Handles

Quick Keys

For scaling objects with a specific amount without having to go into the form, the Quick Keys can be used while dragging one of the scaling handles around the object.

Dragging an edge handle, a single value is expected to determine the amount of change in that direction. This can be a relative value or an absolute value.
Draggina a corner handle, two values are expected with the new width and height of the object. Alternatively, a single value followed by S to scale relatively.

See Quick Keys shortcut table for a list of available actions.

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

Use Coordinates

This sixth option allows you to precisely specify the position of the Pivot Point using the X and Y edit boxes. 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.

Angle

The Angle edit box allows you to specify a precise rotation angle to apply to your selection. Click the Apply button to rotate your selection by the value in this box.

Note:
A positive angle results in a counterclockwise rotation

A negative angle results in a clockwise rotation

Rotate Interactive

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:

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

Quick Keys

For rotating objects with a specific amount without having to go into the form, the Quick Keys can be used while dragging one of the rotation handles around the object.

See Quick Keys shortcut table for a list of available actions.

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 Close button to accept the changes.

Shortcuts

The Shortcut Keys page describes these and other shortcuts that are used in Cut2D Desktop.

Distort Tool

This tool allows you to bend and flex a vector by manipulating a distortion envelope using Cut2D Desktop's standard node editing tools. You can select one or more vectors and then use one of the three different tool modes to create your initial distortion envelope.

Once the distortion envelope has been created, you can use Cut2D Desktop's 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.

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.

Bounding Box

This option is available if you have a selection of vectors . 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 Cut2D Desktop can use to define a curve, above which the other selected objects will be distorted. The distorted object can comprise one or more vectors .

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.

The other objects in the selection can comprise one or more vectors .

Therefore two examples of valid selections for this operation would be:

• 3 vector shapes and 2 open curves

but not:

• 1 vector shape, 1 component and 2 open curves.

The selected objects will be stretched and squeezed between the two curves that were last in the selection. Neither of the contributing distortion curves in the selection will be altered by the operation.

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 Objects

The different alignment options are grouped into three sections:

1. The first section of icons all work in relation to the material (job size).
2. The second section of icons all work with regard to the selected items.
3. The last section provides options to evenly space the selected objects, or to align them inside the boundary of the last object in the selection.

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:

1. Select the item/s you wish to align / move (use single or multiple selection options).
2. Hold the Shift key down.
3. 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 horizontal center

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

Align vertical center

Align the selected items vertically 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 Top/Bottom

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

There are then 4 alignment options for aligning the selection to the outside edge of the last item in the selection:

Align Outside Left/Right

Align the selected items on the outside 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 between the first and last item in the selection, or, if Inside last vector is checked, within the boundary of the last item in the selection.

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).

The Edit Objects Tool Group

Click on an icon to learn more about it:

Edit Objects

The tools relate to the design elements and objects that you can create and manipulate within Cut2D Desktop, for example vector shapes. This is where you will find the tools used to organize, edit or modify these objects.

The tool group is organized in the following way:

Object Selection Tools

Grouping and Ungrouping

The Measure Tool

Object Merge tools

Trim Objects

Interactive Vector Trim

Vector Validator

Create Fillets

Extend Vectors

Fit Curves to Vectors

Vector Boundary

Joining and Closing Tools

Object Selection Tools

Once vectors have been created within Cut2D Desktop 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:

1. Vector Selection
2. Node Editing
3. Interactive Selection

Vector Selection Mode

Selected from Edit Vectors section.

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.

Node Editing Mode

See Also:
• Node Editing Shortcut Keys

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) 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.

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.

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:

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

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.

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.

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:

Measure Tool

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

It has two modes (please note that the options available in both modes are shown in the image here for convenience of documentation, but they are not normally available at the same time).

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.

Object Merge tools

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.

Weld Vectors

Welds overlapping vectors together to create a new shape which follows the outermost edge of all the selected shapes.

Subtract Vectors

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.

Keep Overlap of Vectors

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

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 the trim tool first select the tool by clicking the icon on the drawing tab. You then must select the objects you wish to be trimmed first and then the object you wish to trim against last. Finally, choose whether you want to clear the area inside the boundary or outside of the boundary.

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

Trimmed vectors using
Clear inside 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.

Group the vectors you want to
use as the clipping boundary

Select the vectors you wish to clip
followed by the grouped boundary,
finally trim use the trimming tool.

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.

The only option on the form 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.

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 Search 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 Stop or Close button, or the cross button on the progress bar slowly:

Issues found so far will be marked.
The close button will close the form after stopping the search.

Marks

Examples of the marks described on the form are shown below:

The markers do not move if you move or delete any vectors while the form is open. Markers are automatically cleared when the Search button is clicked or the form is closed.

Vectors can be edited (and Node-edited) while the form is open as long as a search is not in progress.

Text is not validated unless it has been converted to vectors. There is a note on the form to remind you of this.

The search will stop if 1000 issues are found.

If no issues are found a dialog will pop up saying so to confirm that the search was carried out.

If zero-length spans are found, the Fix zero length Spans button is enabled. Clicking this will remove the zero-length spans and clear their markers.

Each time you run the Vector Validator it may appear to find different results first.
The order that the vectors are validated is random because the process is multithreaded; like lots of workers moving a pile of objects onto a conveyor belt that only holds one object at a time...
Several workers may want to put an object on the conveyor belt at the same time...
The final order depends on which worker got there first, as one worker will wait a little to let another place their object on the conveyor.
Which worker waits, and how fast each worker works, varies randomly because the computer may decide that you moving your mouse around is more important than validating vectors and reassign a worker to draw the mouse for a moment, for example.

Create Fillets

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

Not ready to fillet

Ready to fillet

When the check-mark ✓ is visible, click the left mouse button to fillet the corner.

Angle Before Filletting

Angle After Filletting

As well as conventional radius filleting of corners, this tool includes 2 special types of filleting for corners formed by two straight lines. They will create an overcut shaped area in corners to allow clearance for another piece of material to be slotted into the part without being obstructed by material left by the radius of the tool. Below left you can see a blue piece of material fitted into a normally cut slot, this would fit no further in than the radius of the tool would allow. Below right you can see the same situation with a slot which has the Dog-Bone style corners applied to it which allows the part to fit full depth into the slot.

No Filleting

Accurate fit with Filleting

This is a very useful tool for slot-together furniture designs, model aircraft, dinosaurs etc. Below you can see a part from a slot together dinosaur assembly, on the left is the standard part and on the right is the same part with the T-Bone style fillets added to these slots. This type of fillet needs to be used when the slot is close in size to the tool diameter.

No Filleting

Slots Filleted

Fillet / Tool Radius

This size of this value is used to create the fillet as described for each individual type of fillet below. To create any of these Fillets you need to select the type required, then move the mouse cursor so it is over a corner between two vector spans. If it is a legitimate place to create the fillet then a check mark ✓ will show and the user can click the mouse button to create it. It should be noted that sometimes unexpected fillets will be created if the fillet size is too big for the vector shape. In that case, simply undo the change and repeat the process with a suitable fillet size.

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 After Filleting

Normal filleting can also be used on Bezier and Arc Spans, or a combination of all three span types (Straight lines, Arcs, Beziers) if there is enough space to create a fillet based on the specified Radius.

Arc Span Vectors before Filleting

Arc 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 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 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

Horizontal edges clicked
near the corner

In addition, fillet arcs can be removed by simply clicking on an existing fillet arc. This works even for vectors that have been imported with filleted corners. This feature allows the user to easily change the size of fillets by clicking once to remove the existing arc and then clicking the corner to insert the new fillet. In many cases, by allowing the user to control which side of the corner the 'T-Bone' fillet is placed on means that the fillet can be hidden when the pieces are assembled.

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

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. Below are images that show this effect, the first set show the whole vector and the second show a section of the vector in node edit mode to help show the difference. If the fillet was created recently then it may be possible to use the Undo command to return it back to its original geometry.

Original Vector

Vector with Fillets

New Vector after Removing Fillet

Original Vector in Node Edit Mode

Vector with Fillets in Node Edit Mode

New Vector after Removing Fillet
in Node Edit Mode

Extend Vectors

This tool allows you to extend two vector lines to their common point of intersection. The tool form is rather sparse, but that is because all the action occurs directly in the 2D View.

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.

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 Close 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.

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.

The Curve Fitting function can be accessed from the Edit Objects area of the Drawing Tab, the Edit Menu ► Curve Fit Vectors in the Main Menu or by using the short-cut-key combination Ctrl+F.

Fitting Type...

Circular Arcs

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

The vector before fitting

The same vector fitted with arcs

Bezier Curves

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

The same vector
fitted with bezier spans

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 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. The diagram below shows the curve fitted to two straight lines with the max possible distance between them defined by the Tolerance set. The tolerance is the distance indicated with the red arrow:

The same vector fitted with straight lines

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. The images shown below demonstrate how this works. The first image shows a set of straight lines before curve fitting with the angles shown between the spans. The second image shows this after curve fitting with the Keep sharp corners set with a value of 20°. You can see the two lines which were under the 20° difference have had a curve fitted between them but the other corner which has been retained as the original angle is greater than 20°.

Initial Vectors

Result after Keep Sharp Corners

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.

Vector Boundary

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

You can offset the boundary outwards and optionally create convex or 'Rubber band' boundaries.

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 and Rubber Band together

Edit Picture

The Edit Picture form allows you edit the properties and border around the selected bitmap.

Joining and Closing Tools

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

Join Open Vectors

This icon opens the Join Vectors Form

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

Join/Close vectors 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.

Join/Close vectors 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.

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.

The Offset and Layout Tool Group

Click on an icon to learn more about it:

Offset and Layout

Offset Vectors

Linear
Array Copy

Circular
Array Copy

Copy Object
Along Vectors

This tool group includes tools to create offset versions of existing objects or to layout objects automatically.

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:

1. Select the vectors to offset
2. Select the required direction - Outwards / Right or Inwards / Left
3. Enter the Distance
4. Click the Offset 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 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.

Notes

Square Offsetting a very acute (included) angled sharp corner will result in the corner point being positioned a long way from the original geometry, often off the material or cutting through other shapes in the design. To stop this happening Cut2D Desktop checks that the distance for the new calculated offset point is less than 5 x the offset distance away from the original corner point.

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...

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.

This example shows a sign blank copied to create a 3 x 3 array.
3 Rows x 3 Columns with a Gap of 0.3 inches between each object:

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.

Default Block Symmetry Options

Resulting Pattern

Horizontal Symmetry Applied to Row Above

Resulting Pattern

Row/Column displacement...

Entering values in the Row/Column displacement allows you to move a row or column by the value specified.

Row Displacement of 1

Resulting Pattern

Group Copies

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

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.

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 not selected

Angle

Note: A Negative Step Angle pastes the copies in a counter-clockwise direction.
A Positive Step Angle pastes the copies in a clockwise direction.

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.

Copying Multiple Vectors

The result of one array copy can be used for another to create more complex patterns, this one being used for an engraving. The rotation point has been set by double-clicking the centre grip, then dragging to the desired location:

Copying multiple vectors

Result of Copying Multiple Vectors

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.

To make copies of an existing object, select the item to copy, then holding a Shift key down to facilitate multiple selection, select the vector curve or curves you wish to paste the item along. Make sure the Copy Object option is highlighted and click Copy.

If you wish to create circles, then you simply need to select one or more vectors along which the circles will be created. Ensure the Copy Circles option is highlighted and click Copy.

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

Selected Vectors

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

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.

Layers

Vectors, 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.

There are no specific 'rules' on how to use the layers -there are many ways to organize your design and these are likely to vary between individuals and even between different jobs. The 'meaning', therefore, of the layer organization in any particular project is entirely flexible. Some common examples of layers include:

1. Organizing artwork according to the toolpath strategies to be created.
2. One layer for shapes to be profiled, one for those to be pocketed, one for drilling etc.
3. Coloring different parts of the design to reflect different parts of the finished piece.
4. Hiding or locking geometry used as guides or temporary stages in the construction of the final design.

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.

The Layers Tab makes it very easy to work with complex designs giving quick access to all of the layer control options.

From this tab you view all the layers in your current job and modify their properties (such as visibility and color). You can also create, delete, re-order or rename them.

Most of the commands associated with layers can be accessed by right-clicking a layer in the list, or by clicking on the Pop-Up Menu icon to the right of the layer name.

List Item Command and Icons

Each layer in the list has five elements:

Status
Icon

Layer
Color

Layer
Content

Layer 1

Layer
Name

Pop-up
Menu

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 Color

The color swatch can be used to color all the vectors on a layer. Click on the swatch icon and select a pre-set color from the color selector dialog, or choose More Colors... to create an entirely custom color.

Layer Content

The layer content icon will be grayed-out as an additional indicator that the layer is not currently visible. 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.

Note: To delete a number of layers in one go, first hide all the layers you want to keep
then use any layer's Pop-Up Menu icon to select the Merge Visible command.
All the visible layers will now be merged into a single layer, which can be deleted with a single operation.

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

Click the 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.

Additional Buttons and Icons

Show All / Hide All

The visibility icon to the left of the Layers List heading at the top of the Layers Tab will toggle the visibility of all the layers in the list.
If there are both hidden and shown layers, this icon is shown as a dim lamp:
Clicking the dim lamp will show all layers and change to icon to a lit lamp:
Clicking the lit lamp will hide all layers and change to icon to an off lamp:
More options for setting the visibility of multiple items are available from the Pop-Up Menu for each layer under the Show and Hide menu headings.

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 Bitmap 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...
The dialog for adding the new layer is displayed with options to specify the name and color of the vectors on the new layer and an option to indicate if the new layer should be visible.

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 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.

Toolpath Operations

See Also:
• Toolpaths Overview
• The Toolpath List

Click on an icon to learn more about it:

Toolpath Operations
					Basic Toolpaths
					Toolpath Editing Tools
					Preview, Estimation, Tiling and Saving

Toolpaths

The ultimate purpose (in almost all applications) of Cut2D Desktop is to allow you to generate toolpaths which can be run on a CNC machine to machine the finished part in the material of choice. This requires, at a minimum, some vectors to describe the area to which a toolpath will be limited to. The process for creating toolpath is as follows:

Prepare vectors for machining

Optionally organize the vectors you will be using for machining onto appropriate layers.

Set up the Material

Check the overall material size (Job Setup) to ensure it matches or exceeds the size of the finished product.

Use the Material setup form from the Toolpaths Tab to set the reference Z datum for the part relevant to the CNC machine.

Create the Toolpaths

Work through the toolpath strategy icons you wish to use to machine the job to calculate all the required toolpaths.

Save the Toolpaths for the CNC machine

After choosing the appropriate Postprocessor from the list, the toolpaths can be saved in a format which is ready for the CNC to cut. Depending on the toolpaths calculated and the options the Postprocessor/CNC you are using supports, you may be able to save a single file or it may need multiple files to be saved - one for each tool type.

All the stages will be covered in the supplied Tutorial videos that include Machining. It should be noted Stage 1 is done through icons already covered from the Drawing Tab. Stages 2 to 5 use icons from the Toolpath Tab (on the right hand side of the screen). These will be covered in the next section.

Additional Toolpath Tab Features

Switch to Drawing Tab

Closes the Toolpath Tab (right hand screen form) and opens the Drawing Tab (left hand drawing form)

The pin icon is described in the section: Accessing Auto-hidden tabs

Toolpath Summary Area

When a toolpath is selected from the Toolpath list with no other function being used in the Toolpath Tab a text summary of the toolpaths settings is shown in the body of the Toolpath Tab below the icons. This is a very useful way to recall settings for a toolpath without opening it.

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 Set... button to open the Material Setup form:

Material

Thickness

Enter the thickness of the material being machined.

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 environment the side you are setting up will be displayed in brackets e.g. (Top)

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.

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.

Basic Toolpaths

The basic toolpaths section of the Toolpath Operations icons can be found on the Toolpaths tab, underneath the Toolpath list. It includes the Material setup command, which will often need to be used before any toolpaths are created. This section also includes Profiling, Pocketing and Drilling strategies. The Quick Engrave strategy is a specialist strategy for some engraving machines.

Material Setup

Profile Toolpath

Pocketing Toolpath

Drilling Toolpath

Quick Engraving Toolpath

Inlay Toolpath

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 quality.

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.

Cutting Depths

Start Depth (D)

Cut Depth (C)

Tool

Clicking the Select 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 Edit 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 for Profiling

When a profile 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 profile down to the specified Cut Depth. However, by default Cut2D Desktop 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 profiles 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 of the 2D Profile Toolpath page indicates how many passes will be created with the current settings. The Edit Passes... button 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 Apply.

The Delete button will delete the selected pass.

The Clear All 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 Apply.

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 Cut2D Desktop when it creates profile passes initially. However, the Maintain exact tool pass depth option checked, ✓ Cut2D Desktop 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 Set Passes button to create the resulting set of pass depths in the passes list and diagram.

Machine Vectors...

There are 3 options to choose from to determine how the tool is positioned relative to the selected vectors/s.

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.

Last Pass Allowance

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.

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.

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.

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

3D Tabs option selected

3D Tabs option not selected

This image shows how the Length and Thickness values are used when creating 3D and 2D tabs.

Edit Tabs

Clicking on the Edit Tabs... button automatically opens the 2D window and the Toolpath Tabs form is displayed:

Add Tabs

Constant Number

Calculates the length of each selected vector and places 'X' number of equally spaced Tabs around the shape.

Constant Distance between tabs

This option places a tab at the specified distance around the selected shape.

If placing Tabs at the Distance around the shape results in fewer than the Min. number, the minimum number of Tabs are automatically equally placed on the shape.

If the number of tabs calculated using the Distance around the shape is greater than the specified Max. number, the maximum number are placed at equal distance around the shape.

First tab at machining start point

If checked, ✓ a Tab will be placed at the start point (Green node) of a vector when the option First Tab at Machining Start Point is selected.

Dynamically positioning tabs in the 2D View

Interactive Tab positioning is very easy. Simply place the cursor at the point where the Tab is required and click the Left mouse. To Move a Tab, Click and Drag with the Left mouse button on a Tab to move.

To Delete a Tab, place the cursor over an existing tab and click the left mouse button.

The quickest method for adding Tabs to multiple shapes is to use the automatic option to add 'X' number. The position of these can then very easily be modified by clicking and dragging to move tabs to the 'best positions' and also delete unwanted tabs.

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

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 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.

Additional notes on Profile Machining

Machining Open Vectors

The direction of open vector(s) is very important when using Profile strategies as this is used to determine which side of the selection is the right and left for machining. 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.

The Cut Direction - Conventional or Climb controls which end of the open vector the toolpath will start. Changing the cut direction will reverse the direction of cut.

In the following examples, the vector is the magenta dotted line and the arrowed line is the toolpath:

Profiling the Left of the vector using Climb cutting.

Profiling the Left of the vector using Conventional cutting

Talk to your material and tooling suppliers for details about what is most appropriate for your specific type of work.

Tabs can be added to open profile toolpaths Sharp External Corner options do not apply because identifying the outside / inside of an open shape in ambiguous. Leads cannot be added to open profile toolpaths. Ramps can be added to open profile toolpath.

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.

Pocketing Toolpath

This option opens the Pocket Toolpath form for machining 2D pockets. These toolpaths automatically compensate for the tool geometry - both diameter and angle.

Cutting Depths

Start Depth (D)

Specifies the depth at which the pocket 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 must be entered.

Cut Depth (C)

The depth of the toolpath relative to the Start Depth.

Tool

Clicking the Select 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 Edit 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.

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 clickApply.

The Delete button will delete the selected pass.

The Clear All 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 Apply.

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 sets the passes according to the Pass Depth property of the selected tool.

This is initially the default method used by Cut2D Desktop when it creates profile passes. The step size is varied to try and optimize the number of passes (see above) unless the Maintain exact tool pass depth option is checked ✓.

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 Set Passes button to create the resulting set of pass depths in the passes list and diagram.

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 Desktop 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 Edit Passes... 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.

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.

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

Clear Pocket - Offset Strategy

Clear Pocket - Raster Strategy

Raster Angle

Between 0 and 90°, where 0° is parallel to the X axis and 90° parallel to the Y axis.

Profile Pass

Used to clean up the inside edge after machining the pocket. This can be done either before the rastering (First) or after the rastering (Last). If 'No Profile Pass' is selected, you will need to calculate a profile pass manually to machine the pocket to size.

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.

Offset larger than 50%

Tails to clean out corners

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.

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.

Drilling Toolpath

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 Select... 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 Edit... 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.

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.

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.

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.

Quick Engraving Toolpath

This form is used specifically for calculating engraving and marking toolpaths.

Tool

Clicking the Select 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 Edit 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.

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).

Engraving Tool

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

Example of outline engraving

Fill

A pattern is used to engrave / mark inside the selected text or vectors. There are 3 fill pattern options.

Fill engraving with Offset pattern

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.

Output Options

Select the appropriate postprocessor and Save the Toolpath ready to send to the CNC machine, similar to the Save Toolpath form.

If your machine can be driven using a Windows Printer driver (Roland and Gravograph / New Hermes machines use this technique) it maybe be possible to select the installed printer driver and output toolpaths directly from the software instead of saving an intermediate file.

Checking ✓ the option 'Output direct to machine' enables the Device option which is used to setup the appropriate windows printer driver.

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!

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.

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 option not available is the ability to add sharp Corners as again this 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).

The image shown above shows a Stepped Male Inlay created in 1 inch thick material with a 0.75 inch Step Depth and a 0.3 inch Step Width.

All the other standard Profile options are available for Stepped Inlays except there is no option to Profile Inside or On as this does not apply to this inlay type and this option does not allow the use of either the Corner or Lead functions as these are also inapplicable to this type of toolpath.

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).

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).

Setting Inlay Allowances

Although the radius of the tool is compensated for when using the inlay tool, this in itself will almost always not be enough to ensure the two parts will fit together correctly. The parts will be exactly the same size and so would not fit together without a lot of force which would damage the part or without some kind of post-CNC hand work. Cutting the parts exactly the same size also does not allow for any kind of finish to be applied to either side.

To enable the parts to fit extra material either needs to be cut from the Male side, the Female side or in some applications both. This additional distance is added using the option in the toolpath form to add an Allowance. On the toolpaths which are based on a Profile then this is done with the Allowance Offset (Shown in the image below left - highlighted in red). For Pocket style toolpaths use the Pocket Allowance, (shown in the image below right highlighted in red). When a value is entered it will overcut the selected shape by this distance, this will reduce the size for male parts and increase the hole/pocket for female parts.

The size of the Allowance required will depend on the type of material (how much it may expand or contract between being cut and inlayed), the accuracy of your tooling, the accuracy of your machine and finally any finish you are planning to add to the finished parts (such as paint or varnish which will have a thickness). In most situations where no finish is being applied before the parts are inlayed then an allowance of 0.01 inches (0.25mm) or 0.02 inches (0.5mm) will be sufficient. If you are not sure what value to use then you should experiment with this on a test part to get the correct sizes for your particular setup and application.

In the majority of cases the Allowance is applied to the Female side of the inlay as it is typical to not want to alter the actual vector shapes (the Male side) any more than is required for the tool radius. This means the Hole or Pocket will be cut over-sized to provide the additional allowance for the parts to fit.

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.

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 Selector... 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.

In this example, the dialog has been used to select All Closed Vectors on the layer with the name Pocket.

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.

The Associate with toolpath option will be explained in the next section.

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...

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 Selector dialog 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.

Toolpath Editing Tools

The Tool Database

Edit Toolpath

Duplicate Toolpath

Delete Toolpath

Recalculate All 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.

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.

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.

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.

The 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. The Tool Database is accessed from the Select... button every time you create a new toolpath and allows pre-defined tools and settings (speeds, feeds, stepover etc.) to be selected from a list.

New tools can be added, copied from existing tools, deleted and organized. All of the cutting parameters are stored in the database.

Opening the tool database

To access the Tool Database you can click on the Database icon on the Toolpaths Tab:

Alternatively, select Toolpaths ► Tool Database from the main menu bar.

A window similar to that shown will appear displaying a list of the tools that are currently defined on the left and the parameters for the currently selected tool from the list over on the right. Below this image is a list of all the actions that can be executed from this dialog:

Tool List

The Tool List 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. The Toolpath list is arranged hierarchically to allow you to organize your tools according to common properties or use.

You can click and hold down the left mouse button to drag items up or down in the list. If you drag them into a tool group, they will be placed inside the group.

Tooltip of group hierarchy

When a tool is selected within a toolpath strategy page, the tool name does not always provide enough information for you to know whether the tool's settings are appropriate. It is always possible to click Edit and see the full set of the tool's properties and settings. However, if you hover your mouse over the tool's name, a tooltip will pop-up telling you what the location of this tool was in the tool group hierarchy when it was added to the toolpath strategy. This can be extremely useful for quickly distinguishing between tools in your database that have similar names, but have been grouped according to their properties.

Adding a New Tool

Selecting New... creates an empty tool in the list that can have any user definable name.

Copying a New Tool

Copy adds a duplicate of the selected tool to the list and prefixes the original name with (1). Edit the Name and properties for the new tool and click the Apply button to save the changes to the list.

Deleting a Tool

Deletes the selected tool from the database.

Creating a new tool group

Click on the add New Group button then give your new group a name and press Apply to add it to the database. Click and drag tools from the database over the top of the newly created group icon in the tool database tree to add them to the group. Alternatively, select the group and then click the New... button to create a new tool directly within the selected group.

Importing and Exporting tools

Individual tools or complete tool group hierarchies can be saved to disk using the Export... button. Similarly, you can import previously saved tools, groups or even entire tool databases using the Import... button.

Tool Info

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.

Here you can modify any of the properties of the currently selected Tool or Group. Click the Apply button to save the changes to the Tool List.

Name

Use this field to enter a suitable name to describe your cutters.

Tool Type

Various cutters can be specified in the database.

V-Bit

Engraving

Tapered Ball Nose

Ball Nose

End Mill

Radiused End Mill

Form Cutters

Diamond Drag

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.

Geometry

Diameter

The diameter of the tool in either inches or mm. The tool image will indicate where this dimension is taken from. If you change the tool diameter but do not change the tool name then you will be warned.

Cutting Parameters

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.

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.

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.

Feeds and Speed

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.

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.

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

Ogee

Profile Cutting Strategy with Form cutter

Adding your own custom form cutters

Adding a Form cutter to the Tool Database is straightforward and the procedure is,

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. With the vector Selected open the Tool Database (using the command icon on Toolpaths tab or from the main menu, Toolpaths ► Tool Database In the Tool Database window, click New... Select Form Tool

The selected geometry will be imported and a profile displayed in the window.Give the Cutter a meaningful name and enter the cutting parameters - speeds and feeds etc. Click the Apply button to save the new cutter into the database list so it can be used at any time.

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 and Rendering Settings

The pull-down list offers a range of material types to shade the 3D model. The first entry in the list is 'Use Solid Color' and if this is selected the color for the material can be selected from the color picker form.

See Adding Custom Materials below for adding your own materials.

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 More Colors... 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.

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.

The Preview Control buttons are summarized below:

	Run	Begins Preview Control simulation
	Pause	Temporarily halts the tool in its current position and enables the Stop button so you can exit Preview Control mode
	Single Step	Moves the toolpath on by one tool move.
	Run to Retract	Runs the toolpath to the next retract move, then pauses the tool.
	Stop	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

This command allows you to identify a subset of toolpaths to be simulated, quickly and easily:

Verify that the 3D View is only displaying the toolpath previews of the toolpaths you are interested in.

Click Preview Visible Toolpaths to begin the simulation.

Delete Waste Material

If a profile toolpath is calculated the excess material around the edges of the job can be automatically removed to show the finished job.

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

Adding Custom Materials

Additional materials can be added to the library list by simply copying 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. The location of this folder is different on different operating systems, but as an example for \ProgramData\Vectric\Cut2D Desktopmust be restarted when new materials are added.

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.

Multi-Colored Toolpath Preview

When previewing the effects of each toolpath it is possible to assign different colors to each one. This can be used to simulate the effects of differently painted areas both as a way to verify what is being cut by the toolpaths and also to provide an image than can be emailed or printed for customer approval.

Shaded Preview Image

Finished Sign

The different colors can be set from the Preview Toolpath form - this appears automatically when a toolpath is calculated or can be accessed anytime by clicking the bottom, left icon in the Toolpath Operations area of the Toolpath Tab:

When this icon is clicked (or immediately after a toolpath is calculated) then the Preview form will be shown. The options for defining the fill color are contained in the Machined Area Color area of the form:

Solid Material Color

Before the individual toolpath color fill is covered it is worth pointing out another feature within the preview form. There is the option at the very top of the Material List to select a Solid Color for the surface of the part. Once this is selected the color choice can be made from the drop-down Solid Material Color area. This allows material with a different solid color surface and core to be easily represented.

Machined Area Color

Use Material Color

Checking ✓ this option will use the same color/material for the fill as you have selected for the material itself:

Use Global Fill Color

Checking ✓ this will use the same single fill color for all toolpaths:

Use Toolpath Color

Checking ✓ this will let you select different colors for each toolpath in your list:

To set the color individually, first select the toolpath from the Toolpath List and then click on the drop down arrow next to the color block to show the form:

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:

If you click the option at the top of this form where is says No Fill then this will leave that toolpath in the selected Preview Material Color.

Set All

Clicking the Set All button will set all the toolpaths in your Toolpath List to the currently selected color.
ONLY click this if you want to change all toolpaths to have the same color as you cannot undo this operation.

Using the Multi Colored Toolpath Preview option with 3D toolpaths

When assigning an individual color it will be applied to the whole toolpath. If you are cutting a part in Cut2D Desktop with a number of 3D shapes in it you would only be able to assign different colors to them if they were cut with individual toolpaths. In most cases with 3D parts it would probably be better to create a multi-colored image for a customer by shading the components and saving an image of the 3D model than trying to assign different colors to the toolpath preview. This will also allow the use of not just solid colors but the materials for the different parts.

It is worth repeating with regard to the 3D toolpaths that there is the ability to select the No Fill option from the color choice to keep the toolpathed area in the same finish as the material surface.

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 inaccuracies generally come from the acceleration / deceleration of the machine. If the program tells a machine to move at 200 inches / min along a 200 inch straight line the machine will probably take pretty close to a minute.

If instead of a straight line we ask the machine to cut say a gear wheel with a total circumference of 200 inches, the machine is likely to take considerably longer. This is because the machine will have to slow down to go around the tight curves of gear tooth profiles and will probably never reach its programmed speed before having to slow down again for the next change in direction.

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.

If a job actually takes 6 minutes to cut and the estimate was 3 minutes, the scale factor would be set to 2 (actual time / estimated time = 6/3).

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.

Toolpath Tiling

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.

The Toolpath Tiling Manager

The toolpath tiling form will 'split' the full-size toolpaths into a number of discrete, but precisely aligned, toolpath tiles as soon as you click the Update Tiles button. Any toolpath arcs spanning a tile boundary will remain as arcs after tiling.

While the Tile Toolpaths mode is enabled (using the checkbox on this form) any toolpaths that you save will automatically be divided into tiles.

The top section of the tiling form allows you to set the type of tiling you require (see below for more information) and the appropriate settings for each tiling strategy.

The lower section of the tiling form allows you to select and activate each of the tiles. The currently active tile can be previewed in either the 2D or 3D View.

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. Cut2D Desktop specifically 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. You should pay particular attention to the fact that this overlap can take the toolpath outside of the tile boundary - this is necessary to ensure that 2.5D toolpaths, in particular, form the correct shapes at the tile edges.

An independent toolpath tile preview in the 2D View. The light red areas indicate the current overlap settings for this tile.

This image shows the same toolpath tile's 3D preview, positioned relative to the machining origin. You should note that the tool will machine negative, as well as positive, relative to its origin in this case. You must allow for this necessary effect when setting up your material and origin for machining.

When you come to machine these tiles you should take care to allow for the overlap distance when setting your machining origin on your material. Internal tile toolpaths can machine negative, as well as positive, relative their origin.

The currently active tile can be set directly from the 2D View by double-clicking on the background of one of the indicated tile regions.

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 origin.

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.

Saving 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 from Cut2D Desktop is to:

1. Select the toolpath to save from the Toolpath List
2. Click on the Save option and the Save Toolpaths form is displayed.
3. Select the correct Postprocessor for the CNC machine from the pull-down list
4. Click the Save Toolpath(s) button
5. Enter a suitable Name and click the Save button

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,

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 Save Toolpath(s) button Enter a suitable Name and click the Save 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.

The Toolpath List

The Toolpath List is located at the bottom of the Toolpath Tab (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.

The up and down arrow icons to the right of the window allow the user to move a 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.

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.

Resizing the Toolpath List

The toolpath list can be resized by clicking on the divider between the toolpath list and toolpath commands area and dragging.

Main Menu

Clicking on any of the options on the title bar (File, Edit etc.) will result in a drop-down menu appearing with choices related to that topic.

Many of these are just an alternative way to access functions also accessed through the icons. However, there are a few commands that are unique to the Drop Down menu. Each menu and its contents are discussed later in this section of the manual.

Only unique items which do not have an equivalent icon that has already been discussed in the manual will be dealt with in detail.

File

	New	Creates a New Cut2D Desktop job.
	Open...	Opens an existing Cut2D Desktop job
	Close	Closes the current file but leaves the software running
	Save	Saves the current Cut2D Desktop 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 PhotoVCarve or Cut3D Toolpaths...	Import a toolpath file created in another Vectric application, such as, Cut3D or PhotoVCarve.

Export

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 OK button on the dialog will store the settings without printing immediately.

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 Print... button to begin printing the document directly from the Print Preview page.

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.
	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 Help Menu ► Post-Processor Editing Guide.
	Document Variables	Opens the Document Variables dialog.
	Snap Options	Opens the Snap Options dialog. See Rulers, Guidelines and Snapping for more details.
	Options	Opens the Program Options dialog to allow the customization of certain aspects of the program.

Selection

Toolpaths Menu

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

Tool Database Opens the Tool Database Dialog.

Recalculate All Toolpaths Recalculates all the Toolpaths in the part.

Toolpath Drawing ► Opens the Toolpath Drawing Pop-up Menu.

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

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.

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 Shortcut key for this is F5. 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 at the end of the 2D Design part of this manual. Opens the Guide Lines Pop-up 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.

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 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.

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.

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

Page
DownTile Windows Horizontal: Tiles the 2D and 3D View Horizontally, 2D View at the top and 3D at the bottom.

Page
UpTile 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.

Help

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

Keyboard Shorcuts: Displays the Shortcut Keys available in the software.

Video Tutorial Browser...: Access the tutorials

What's New: See a summary of the new features added in major updates.

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

Enter License Code The license details provided when you purchase Cut2D Desktop

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 theVectric User Portal in your Web Browser if you have an Internet Connection. Download software installation files and activation codes included with the software.

Post Processor Editing Guide: Opens a PDF manual 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 Desktop 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 Desktop... This window displays the version of the software being used, to whom the software is license and the type of license.

Right Mouse Click menus

Clicking the ►RIGHT hand mouse button in different places in Cut2D Desktop 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 document details some of these areas and the menus that you will see when RIGHT mouse clicking.

2D View Right Mouse Menu

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.

The Copy to Layer, Move to Layer and Move to Sheet 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.

Span Editing Menu

If the currently selection mode is set to Node Editing, one of 2 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 in the selected vector in the 2D View. These menus have functions in them that correspond specifically to this selection and position. The menu below will appear when the cursor is over the 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. All these have corresponding Short Cut keys (shown to the right of the command in the menu) which can be selected from the key-board 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 the Node of a vector in Node editing mode. You can see a variety of choices to convert the span to Delete the Point, Smooth it, Cut the vector at that point or change the point to be the Start Point on the vector. From this menu you can also close the vector, Exit the node editing mode and lastly see and edit the exact XY co-ordinate position of the node by selecting Properties. All these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the key-board 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.

Component Grayscale Menu

When a Component Grayscale is the selected item and Object Properties is selected it opens the Bitmap Properties slider, allowing you to change the fading of the grayscale component. Two other options are also available on the Right mouse click menu for a selected Component Grayscale. Move to Front and Move to Back. Clicking Move to Front will make the selected Grayscale appear over all the other Grayscales on the same layer so you can see the selected one more easily. Move to Back will send the selected one behind all the others on the same layer so that it is easier to see all the other Grayscales in the part.

Component Menu in the 3D View - Selected Components

When a component(s) is selected in the 3D view you can RIGHT mouse click and make changes to that selected component(s). You can check the combine mode of a component. You can Unselect a single component or Unselect All depending on how many components you have currently selected. You can hide and delete a component. You can open up the properties form for that component and you have the option to move the selected component(s) to an existing or new Level.

If you choose New Level you will be presented with the box below, where you simply add in the name for the new level and choose a combine mode from the dropdown menu.

Component Menu in the 3D View - Non Selected Components

When you RIGHT click on a component without selecting it first the menu will display the names of the components that are positioned at the point your cursor is within the job space. Selecting the name of the component will select it and open up the Properties form for that selected component.

Clipart Menu

When you RIGHT click on a piece of clipart in the clipart tab you have the option to import it to a new or existing level in your job. This will position the object in the center of the workspace and add it to the top of the list of Components on the selected Level or if you choose New Level will allow you to enter a name and Combine Mode.

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 and 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.

Glossary

2D View

Shows the workspace defined when you create a new file. This is used to control the XY layout of vectors and bitmaps. Typically you select an item from this view by clicking on it or dragging a box around it with the mouse. To move it you can click a selected item a second time to go into Transform mode. Some items when double clicked will open a form relating to the object and many have functions related to them displayed when you right mouse click over them.

Group

When you want to manipulate a number of objects together you can Group them. This is a temporary operation to ease the selection, movement, scaling, and rotation etc. of several objects at once. It is reversed by Ungrouping.

Ungroup

Separates a set of Grouped Objects so that they can be manipulated independently again.

File

Generic name most often used to describe a complete Cut2D Desktop project (CRV file) which contains all the 2D and Toolpath information in a single saved file - also sometimes referred to as a Part.

Short Cut Keys

Keys on the keyboard which will activate certain commands when pushed. Example F4 to activate the Snapping Options Dialog. You can find a full list of all the Shortcut Keys in the online reference manual in the Frequently Asked Questions section.

Vector

A 2D object represented by lines, arcs or curves.

Frequently Asked Questions

Navigating this Document

Click ► Arrow Triangles to open a fold in the document.

Open all folds before printing or searching for text in this document.

[Close All Folds]

[Open All Folds]

General Questions

► Where can I get Help?

If you need assistance when using the software these are the primary places to look:

1. Program Help File: From the Main menu select Help
2. Video Tutorials: These are supplied on the installation DVD or can be downloaded from the Vectric website.
3. User Forum: The Vectric user forum at www.vectric.com/forum is a very useful resource for information on Cut2D Desktop along with materials, cutters etc. and also to share knowledge and experiences.
4. Email Support: The Vectric Support Team at support@vectric.com
5. Support Website: http://support.vectric.com/ provides access to Frequently Asked Questions, Training Materials, Updates and Upgrades, Gadgets and Free Projects for some Vectric software.

► What file formats can be used?

Cut2D Desktop will open files that have been saved in the following formats:

Vectors

File Suffix	Format summary
DXF	Drawing Exchange Files from CAD systems
EPS	Encapsulated Postscript from Adobe Illustrator and Corel Draw etc.
AI	Adobe Illustrator
PDF	Portable Document Format for industry standard print data
SKP	SketchUp software files

If the designs are being prepared with software such as Corel Draw or Adobe Illustrator we recommend that you convert the vector geometry and text to curves and switch off all patterns or color fills before exporting, preferably as an EPS file.

Images

File Suffix	Format summary
BMP	Windows Bitmap Format
JPG, JPEG	Compressed format commonly used for digital photographs and websites
GIF	A common web format, usually with a limited number of colors
TIF, TIFF	A compressed format, including a 16-bit version
PNG	More recent format with a good range of properties

3D Models

File Suffix	Format summary
STL	CAD orientated 3D design packages and scanning systems
DXF	Many CAD systems - data must consist of meshes or triangles
3DS	3D Studio and many other animation orientated packages
OBJ	Wavefront
SKP	SketchUp software files
V3M	VectorArt 3D clipart models

► What are the limitations of the Trial Versions

The Trial Versions will let you use all functions within the software with the exception of saving the toolpaths and performing some Export functions.

The Pro Versions of the Trials also do not allow you to use additional Gadgets.

There are a collection of special "trial version specific" files made available for each program that are setup so you can save the toolpaths from them and verify compatibility with your CNC machine by actually machining the samples.

For Aspire, VCarve Pro/Desktop and Cut2D Pro/Desktop these are found in the Getting Started Tutorials from the Video Tutorial Browser. For more information about these tutorials please use the link for "How do I use tutorials in the Trial Edition?".

You can also access the Trial Projects from the option Evaluation Files to Machine found on the first screen of the Trial.

Cut3D comes with a set of Trial files that are accessed from the trials start screen.

PhotoVCarve can work with any photo image however restricts the toolpath output by applying a watermark to all images.

► What are the minimum requirements for my PC to run Vectric software?

The Aspire, VCarve, Cut3D, PhotoVCarve and Cut2D software products will all run on virtually all home PC's and do not require any special hardware or graphics card.

Aspire, VCarve Pro/Desktop and Cut2D Pro/Desktop software is 64Bit and 32Bit, and will work on both 32bit and 64bit Operating systems.

Cut3D and PhotoVCarve software is 32bit, and will work on both 32bit and 64bit Operating systems.

Vectric Software does not support Windows 8RT as this is not a full edition of Windows.

The minimum PC specification for Aspire and VCarve Pro/Desktop is:
Computer:	2 Ghz multi Core CPU 2Gb RAM with Windows XP(SP3), Windows Vista & Windows 7, 8, 8.1 or 10 300 Mb Disk space (Program) USB drive required for USB Media Pack if purchased. 7.7GB Additional disk space required if you wish to store the tutorials and clipart supplied, on your hard drive.
Display:	1024 x 768 Graphics display
Operating System:	Microsoft Windows XP (SP3), Vista, 7, 8, 8.1 or Windows 10 with 2Gb RAM

The minimum PC specification for Cut2D Pro/Desktop is:
Computer:	2 Ghz CPU 2Gb RAM with Windows XP(SP3), Windows Vista, Windows 7, 8, 8.1 or 10 250 Mb Disk space (Program) USB drive required for USB Media Pack if purchased. 2GB Additional disk space required if you wish to store the tutorials and clipart supplied, on your hard drive.
Display:	1024 x 768 Graphics display
Operating System:	WindowsXP (SP3), Vista, Windows 7, Windows 8 or Windows 10 with 2Gb RAM

The minimum PC specification for Cut3D and PhotoVCarve is:
Computer:	1 GHz Pentium 4 512 Mb RAM 60 Mb Free disk space CD Drive
Display:	1024 x 768 Graphics display
Operating System:	Windows XP (SP3), Windows Vista, Windows 7, Windows 8 or 8.1, Windows 10
Other:	A PDF reader program (such as Adobe PDF Reader) is required to read the documentation.

Note: The Intel 82810 & 82815 integrated graphics cards must be set to run in 16 bit color mode.

► How many computers can I install my Vectric software on?

Vectric's license allows any of our software programs to be installed on up to 3 PC's for a single user.

If access to any one of the computers is shared with work colleagues, or anyone who is likely to access the software, then the software must only be installed onto one computer.

► Do you have educational pricing for Vectric Software?

All Vectric products are available for purchase by registered educational establishments and we have very special pricing available for classroom licenses.

Please send an email to This email address is being protected from spambots. You need JavaScript enabled to view it. for further information.

Educational purchases cannot be made via the Webstore front, only via the sales team.

► Can I run the Trial Version in a non-English version?

Yes, for Aspire, VCarve and Cut2D, the Trial software is available in alternative languages through our Spanish website.

While the website is in Spanish, the Trial installers have our full range of International languages included.

For PhotoVCarve and Cut3D, the Trial Versions are available only in their English version.

If you are interested in what language versions may be available for purchase, contact This email address is being protected from spambots. You need JavaScript enabled to view it. and we will help you.

► Why do I receive an error opening recent files?

If you receive a warning similar to this:

e.g. File Missing

The file you are trying to open has either been deleted or moved to another locaton on your computer.

Click OK, and use "Open an existing file" to manually locate your file.

---

► Why do I get "An unknown error occurred while accessing an unnamed file" when saving to a network location?

Errors when saving across a network is likely caused by minor faults in a network connection.

It is more reliable to work from the local drive, and less likely to result in lost or corrupted files.

Should you encounter this error when saving, save your projects to a local destination and then back them up to your network accessed storage once completed.

► Where is the Vectric Files folder?

In Windows Vista, 7, 8 and 10, the Vectric Files folder is most easily located using the Documents item under Libraries in Windows Explorer. Following the default installation, the folder is: C:\Users\Public\Documents\Vectric Files

In Windows XP the same folder is C:\Documents and Settings\All Users\Documents\Vectric Files

► Where do I look to find the Tool Database on my PC?

Start the program and use the File Menu ► Open Application Data Folder. This will open a new window showing all the program's support folders. Select the ToolDatabase folder to find the Tool Database file.

► Where do I look to find the Post Processors folder on my PC?

Start the program and use File Menu ► Open Application Data Folder. This will open a new window showing all the program's support folders. Select the Postp folder to find the Post Processors.

► Where do I look to find the Gadgets folder on my PC?

Start the program and use File Menu ► Open Application Data Folder. This will open a new window showing all the program's support folders. Select the Gadgets folder to find the Gadgets.

► What is the latest software version available?

To check which version of the software you are running, please run the software and click the Help Menu ► About....

If you are not running the latest major release version as above i.e. you are using Aspire 8 instead of Aspire 9, then you may want to learn more about the new and exciting features that have been added to your product.

You can check out the latest enhancements as well as our affordable upgrade options by visiting: http://support.vectric.com/upgrade

If you are running an older version then you may be entitled to update to the latest minor release of that software. You can view all available updates by visiting: http://www.vectric.com/support/program-updates.html

► What is the difference between Updates and Upgrades?

Each version of the software comes with a Version Number.

For example: VCarve Desktop V8.012

In this example, VCarve Desktop is Major Version 8 and Minor Version 0. The following 2 numbers then give it as Patch number.

When you do a software Upgrade, you are doing a transfer from one Major Version of the software, to another Major Version of Software. These Upgrades are almost always done via the Vectric Store Upgrade Page, or via an email notification to your registered email address.

For example: This could Upgrade VCarve Desktop v8 to:-

Aspire v8 or higher when released

VCarve Pro v8 or higher when released

VCarve Desktop v9 or higher when released

When you do a software Update, you are updating the Minor software version and the Patch number.

Currently all Vectric customers are able to download the latest Minor Version update for the Major Version they own.

For example:-

Aspire v8.007 ► Updates to Aspire v8.012

VCarve Pro 7.0 ► Updates to VCarve Pro 7.514

All Software Updates and Patches can be downloaded within the software by going to Help Menu ► Check For Updates. This will begin the download of the latest available Updates for your software, and will require an internet conenction. For Manual Patching visit the Software Updates Page to download your patch. If a manual patch does not automatically find the software version when used, it is likely that you do not have the correct Update for your Major Version.

Summary:-

Major version releases include new Major features for the software, such as new tools and important features. These are usually Paid Upgrades.

Minor Version releases include some smaller new features or adjust existing features to make them easier to use. These are usually free Updates.

Patch releases include minor tweaks and fixes to ensure existing features work as intended. These are always free updates.

► What are Gadgets?

A Gadget is an external add-in program that performs a specific task for our Aspire, VCarvePro and Cut2DPro products only.

A section of our website is dedicated to Gadgets: http://gadgets.vectric.com.

► What is the Vectric License Transfer Policy?

Can I transfer my Vectric software?

Unlike the vast majority of software companies, Vectric does allow the original purchaser of a software licence to transfer it under certain circumstances, and subject to a licence transfer fee. However this is NOT an unrestricted right of transfer, and Vectric reserve the right to refuse to transfer the licence, at its sole discretion, if it reasonably believes there is evidence of the license conditions having been broken. If you upgrade a product from say Version 4.0 to Version 5.0, you still only own one licence and that is now for Version 5.0: you no longer have a valid licence for V4.0 and so the licence for the older version obviously cannot be transferred.

Software licence purchased directly from Vectric or an authorised Vectric partner

If you have purchased a single user license directly from Vectric or one of our authorised partners, we would usually allow you to transfer the single user license to another individual or company, subject to the licence conditions having been adhered to and the payment of a licence transfer fee (currently $50).

You cannot transfer a license that you have not directly purchased (i.e. one that has been transferred to you, from a previous licence holder). The original purchaser of the software licence can transfer it once, but subsequent owners cannot.

If you upgrade a product to a more expensive one, you cannot subsequently transfer the initial product licence. e.g. if you upgrade VCarve Pro to Aspire, the VCarve Pro licence has been 'traded in' against the Aspire licence and you no longer have a licence for VCarve Pro.

Software licence transferred from a previous original owner

If you have obtained a licence from a previous original owner, you cannot subsequently transfer that licence to a new owner, unless the software licence was originally bundled with a machine, and you are transferring the machine along with the licence (see section below for this case). The transfer rights for the software are only available to the original purchaser of the software from Vectric or one of our authorised partners. If you are planning to buy a 'used' licence of Vectric software from somebody, it is essential that you contact Vectric first via This email address is being protected from spambots. You need JavaScript enabled to view it. to ensure that the licence in question can be transferred.

Software licence originally bundled with a machine tool

If you received Vectric software bundled with a machine tool from an approved Vectric partner, you may transfer the software along with that machine tool, providing that you have not used the license to upgrade to a different product. This applies even if you are not the original purchaser of the machine.

If you have upgraded the software, the upgraded product would need to be transferred along with the original media supplied with the machine. You do NOT have to transfer the software licence when you sell the machine, but the new owner of the machine will need to purchase their own copy of the software if they wish to use it in this case.

Educational Software Licence

Educational classroom licenses cannot be transferred.

---

Please email details of any license transfer requests to This email address is being protected from spambots. You need JavaScript enabled to view it.

► I Need to Email Support

If you ever require help with your project, in particular any project that involves issues with your toolpaths and generating toolpaths we will need to see the original project files to be able to give accurate advice.

When preparing to email This email address is being protected from spambots. You need JavaScript enabled to view it. to request assistance, please check the following points.

• Make sure you list the exact name of the Post Processor you are using to create your toolpaths. There are many Post Processors with similar names and they can often be mistaken for each other.
• Once you have created your toolpaths, save a copy of your project to send to us. It can be very helpful if we can see your toolpaths exactly as you created them in the project.
• If you are having trouble with a particular toolpath and its cutting results, send the Gcode file you have generated along with your project.
• If you are experiencing a crash with the software, and can replicate it, save a copy of the project right before the crash and detail the steps you take to make it crash. This will provide the steps we need to fault find the cause of the issue.

It can help to compress (ZIP) your files. This will make them smaller to send via email, meaning you will spend less time uploading them.

Lastly, always send your support requests from the email address you registered your software from. This will reduce any delay while we confirm your registration.

► How do I use tutorials in the Trial Edition?

1. Open Trial software
2. Click Tutorial Video Browser in left hand panel
3. Click View Tutorials under By Catagory
4. Click Wing Spar under the Getting started heading
5. Click Download Files
6. Open downloaded installer and run it, following on screen instructions
7. Go back to Internet browser witht he Tutorial Window and press F5
8. This will change the "Download Files" to "View Files"
9. Click on "View Files" and you will be able to open the CRV files which contain toolpathing you can export with the appropriate Post Processor for your machine. Please be sure to edit the existing toolpathing to correct the tool settings and Cut depth to be suitable for your machine to avoid creating commands that may damage your machine and toolbits.

► How do I Uninstall Vectric Software?

This Article applies to all Vectric products and versions.

On installation, all Vectric products will create a listiing in the Windows Programs and Features control panel applet ('Add or Remove Programs' in older versions of Windows).

Windows 8, 8.1 or 10

1. Open the Windows Start menu (Windows Key). From the Start screen, start typing Control Panel (the search should autofill after a few characters).
2. Click on Control Panel from the Apps search results, in the opened Control Panel window, select Programs and Features
3. In the Programs and Features window, you will see the Vectric product listed amongst the other applications installed on your computer. Select the Vectric application that you wish to uninstall and click on the Uninstall button.

Windows Vista or 7

1. Open the Windows Start menu (Windows Key). From the Start click on Control Panel
2. Depending on your view options click either on Uninstall a program or Programs and Features
3. In the Programs and Features window, you will see the Vectric product listed amongst the other applications installed on your computer. Select the Vectric application that you wish to uninstall and click on the Uninstall button.

Windows XP

1. Open the Windows Start menu (Windows Key).
2. From the Start screen, click on Settings then click on Control Panel. In the Control Panel window click on the Add or Remove Programs applet.
3. In the Add or Remove Programs window you will see the Vectric product listed amongst the other applications installed on your computer. Select the Vectric application that you wish to uninstall and click on the Change/Remove button.

► How do I find which version of the software I am running?

Select Help Menu ► About Cut2D Desktop... from the Main Menu and a dialog window will open that shows the exact version you are using.

► How do I find and install an update when a newer version of the software is available?

Select Help Menu ► Check for Updates from the Main Menu and if this tells you an update is available, follow the prompts to download and install the update automatically.

You can also download the latest versions from the Customer Portal.

► How do I download my free Clipart?

New Version 8.0 and higher sales of Aspire and VCarve Pro/Desktop come with a collection of free Clipart files to use in these versions of the software.

Due to their size they are not included with the main software download.

To access them you can log into your Vectric Portal account and click on the View Downloads for your software.

This will load a page with your software download and licence details, and when you scroll down the page you will see all of your Clipart links to download from.

Some of these are large downloads (more then 200MB) and will take some time to download depending on your interent connection.

Alternatively, you can install the Clipart from your Media DVD if you selected this option when purchasing the software. If your software was bundled with your CNC machine on purchase, you will have a Media DVD. Load the DVD into your DVD drive on your PC and select the option to install the Clipart and follow the on-screen instructions.

► How do I add new material image files to the available list?

From Aspire 4 / VCarve Pro 7 onwards you can add new images to the Material Images folder in your Vectric Files folder.

In Aspire 3.5 / VCarve Pro 6.5 or earlier you will need start the program and use the File Menu ► Open Application Data Folder.... This will open a new window showing all the program's support folders. You can add new material image files to the Bitmap Textures folder.

You will need to restart the software for your new image files to appear in the material drop-down lists.

► How do I access installed Video Tutorials?

For Version 8.0 and above, you can access the tutorials through the tutorial video browser which is accessed from within the program when you first start the software. There is a link to it on the left side of the interface under the Recently Opened Files section. If you have a disk or USB stick then you can download the tutorials to your hard drive where you can access them in your Vectric Files folder on your PC.

For VCarve Pro 7.0 and Aspire 4.0 there is an option to install the video tutorials from the Installation Media. Choosing this will copy all the tutorial videos and files into the Tutorial Files folder which is located under the Vectric Files folder on your PC.

The installation will also create a shortcut icon for your default Web Browser on your Desktop which will be labeled with the appropriate software name and version. Clicking on this will open a Tutorial Browser that can be used to navigate the different sets of tutorials and access the videos and related files.

► How can I compare the features of each Program?

When trying to decide which Vectric program will best suit your needs, you can use the Software Comparison Chart.

If you still need more information, asking on the User Forum should get you some answers from experienced users and you can download the Trial Versions of the programs and work with your designs for free.

► Dropbox and File Sharing Folders

While Dropbox and other File sharing distribution methods are helpful for sending project files between friends and colleagues, for best practices we recommend having a local folder on your Hard Drive to save your .CRV and .CRV3D Project files from Aspire/VCarve/Cut2D, before then copying them from this folder into the special Dropbox (or other Shared) Folder.

This is because with the way File sharing works, if a friend or colleague accesses your file when you go to save (Or the system Syncs the file at that time) then it can lead to file corruption and lost data.

Saving the Project file directly to your local Hard Drive prevents this from happening, and allows you to then safely copy and paste the correctly saved file to your Shared Folder.

This has the added advantage that is someone edits your shared file, you can still access the original saved on your local computer if required.

► Double Clicking loads older version

After updating to a new version, files (.crv / .crv3d) still open in the older version when double clicked.

This can occur if the previous major version of a product is not uninstalled before the newer version is installed.

Windows fails to correctly update the Windows Registry keys to open the newer version when requested.

To correct this, a couple of steps need to be taken:

1. Uninstall the previous version (be sure to back up any custom Post Processors or Toolbit database settings first if you have not already transferred them to the new version)
2. Reinstall the New version.

Now check to see if this has managed to correct the issue in Windows by double clicking one of your .crv / .crv3d files. This should allow the New Version to over write the effected Registry keys now that the original versions software is no longer installed.

This reinstallation must be done with a computer account that has full write accesses rights to the Windows Registry.

► Can Vectric software run the CarveWright machine?

None of the Vectric products can directly run the CarveWright machine, however:

• Aspire can be used to create and export 3D Models in STL format, which can then be imported into the CarveWright software using their optional STL Importer.
• A 3D model may be saved from Aspire as a Grayscale height-map image that can then be opened into the CarveWright software, which will automatically recognize the grayscale as a carvable relief model.
• In addition, you can export vector drawings as DXF format, which can be imported into the CarveWright software via their optional DXF Importer. You can find more information on the STL and DXF Importers on the CarveWright website.

► Can I open the files created in the Trial Version of the software into the full version?

Yes, but only on the same computer that the Trial Version was installed on.

Once you have opened the files in the release version and resaved them, you can then open them on any computer running the program.

If you do have files that were created in the Trial Version that you need to keep and use, it is a good idea to open and save them as soon as possible after installing the release version as any problems or hardware changes to the PC could prevent the program from opening those files from the Trial Version.

2D Design - Vectors & Images

► Can I open Corel Draw files?

Yes, Corel Draw files can be opened in Aspire, VCarve and Cut2D but not directly as CDR files. The design needs to be exported from Corel using the EPSfile filter, which is very easy to do:

1. Select the required lines / shapes / geometry in Corel
2. Remove any Fill Patterns and set the Line Thickness = Hairline
3. From the File menu select Export
4. Tick the option Selected only
5. From the Files of Type select the EPS - Encapsulated Postscript option
6. Click the Export button
7. Click the option to Export Text as Curves

The file can now be opened / imported and toolpathed in Aspire, VCarve and Cut2D.

► How can I change the Job / Material Size?

The material size for a job can be changed at any time by selecting Edit Menu ► Job Size and Position or the Job Setup icon in the Drawing Tab to open the Job Setup form.

The Units, Width, Height, Thickness and Z Origin can all be changed on this form.

The origin for the job can be specified to be any of the four corners or the middle of the job, and an offset distance can be entered to move the selected origin by the required X and Y distance.

Checking Center vectors in material will automatically reposition the vector design central to the new material size.

Important:

If the Z Origin is moved, all calculated Toolpaths MUST be recalculated.

We recommend that you always recalculate toolpaths whenever the material has been changed. This will ensure the toolpaths cut correctly on the CNC machine. This can be done very quickly by using the Recalculate All Toolpaths icon: in the Toolpath tab.

► Will the Vectric programs allow mathematical equations to be calculated?

Where appropriate, numerical edit boxes support simple math calculations.

Instead of working out a value, you enter an expression directly into the edit box using Special Calculation Characters as needed and then press the = (equal) key.

As soon as the = key is pressed, the program will evaluate the expression and fill the edit box with the results.

► Why group vectors?

The ability to group vectors is a big advantage for the user. Grouping takes two or more vectors and creates a single object (group) that can be moved around and manipulated without the individual vectors changing their position relative to each other.

At any time, Grouped vectors can be ungrouped to allow changes to be made.

► When moving a vector using the Move Selected Objects tool, what is the difference between Absolute and Relative modes?

Absolute mode will move a vector or component using the drawing coordinates.

For example, you have a circle with its center at X = 3, Y = 7.5 and you want to move it to X = 6, Y = 4. Select the circle and press M, the shortcut key for the Move Selected Objects tool, then select Absolute and the center anchor point. Change the value in the X input box to 6, the value in the Y input box to 4 and select Apply to perform the move.

Relative mode will move a vector or component from its current position by the number of units entered in the X and Y input boxes.

Using the above example, you would select Relative and enter +3 in the X input box, -3.5 in the Y input box, then select Apply to perform the move.

Note: An anchor point is not required in Relative mode as the entire shape will move the same number of units in X and Y based on its original position.

► What do the different line colors mean?

Selected vectors are drawn in .
Usually, selected vectors are drawn as dotted lines but Grouped vectors are drawn as solid lines.

The top three lines are selected.
The top two are grouped together.
The bottom line is not selected and will be the color of the layer it is on.
See the Layers section for more.

► What is the difference between Ungroup back to original objects layer and Ungroup onto groups layer?

Vectors remember what layer they were originally created on, even after being grouped. If you need to ungroup them, you have two options.

• Ungroup back to original objects layer: After ungrouping, the vectors will return to the layer they were created on.
• Ungroup onto groups layer: After ungrouping the vectors will stay on the current active layer.

► What is an open or closed vector?

Vectors can be open or closed.

• An open vector is a vector that does not join back with itself and the easiest example to visualize is a line.
• A closed vector is one that joins with itself to form a shape with good examples being a circle or rectangle.

Sometimes you can have what looks to be a closed vector but is in fact an open vector. This can cause problems when setting up toolpaths, as some toolpaths treat open vectors different from closed vectors.

There are two quick ways to find whether a vector shape is open or closed:

1. You can use Edit ► Select All Open Vectors and see which ungrouped vectors become highlighted or...
2. Select the vectors you want to check and use the Join Open Vectors tool: This tool will tell you how many of the selected vectors are open and how many are closed.

► What is a node and how do I use them?

One of the fundamental building blocks in the program are vectors and vectors are two or more nodes joined by lines, Bezier curves, Arcs or a combination of these.  The position of the nodes, whether they are smooth or not and the position and strength of their associated control points will dictate the path (shape) that the vector follows between nodes.

You can see and use nodes after selecting a vector and pressing N to enter Node Editing mode.

Node Editing is a very powerful feature, allowing the user to precisely modify a drawing, troubleshoot problems with vectors, and help setup some types of toolpaths.

► What fonts come with the program?

The program offers a selection of Single-Line fonts suitable for efficient engraving as well as being able to use all the Windows True-Type Fonts that are installed on your PC.

The font is selected in the Forms that create Text:

• Create Text
• Auto Layout Text

► What are the Special Calculation Characters?

See Also:
• Shortcut Keys

In addition to performing calculations using numbers with standard math operators (+,-,*,/,^, etc.), the program recognizes several Special Calculation Characters to simplify common operations. These are shown in the table below with examples of how they are applied.

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=	Circumference 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)

► What are the Node Editing Short-cut Keys?

See Also:
• Shortcut Keys

Node Editing is a very powerful feature to assist you when working with vectors. You enter Node Editing mode by selecting the vector you want to node edit and then either pressing N, the shortcut key or using the Node Editing icon.

Shortcut key	Description
I	Insert a Point
D	Delete Point / Span
S	Smooth / Unsmooth Point
C	Cut Vector opens the vector
B	Convert span to Bezier
A	Convert span to Arc
L	Convert span to Line
P	Makes the selected node the Start Point for machining
X	Displays a single node's X and Y location properties
X	Changes the X co-ordinate position of selected nodes to match the position of the first one (when more than one selected)
Y	Changes the Y co-ordinate position of selected nodes to match the position of the first one (when more than one selected)
H	Enter horizontal mirror mode (press again to exit)
V	Enter vertical mirror mode (press again to exit)
Right mouse click	Opens context sensitive menus
Ctrl + Z	Edit Undo
Ctrl + Y	Edit Redo
Ctrl + C	Copy the selected vectors
Ctrl + V	Paste the selected vectors
Ctrl and Drag	Pastes a copy of the selected vectors each time the left mouse button is released.
Ctrl + X	Cut the selected vectors
Alt and Drag	Moves the object either horizontally or vertically aligned with its original position
Ctrl + Alt and Drag	Creates a copy of the original object horizontally or vertically aligned to its original position
Ctrl + N	Create New file
Ctrl + O	Open an Existing file
Ctrl + S	Save file
Ctrl + I	Import file
Page Up	Vertically tiles the 2D View and the 3D View window so you can see them both simultaneously. Currently Selected window is on the left - typically best to select the 2D View first when doing this.
Page Down	Horizontally tiles the 2D View and the 3D View window so you can see them both simultaneously. Currently Selected window is at the top - typically best to select the 2D View first when doing this.

► What are the Keyboard Short cut Keys?

Cut2D Desktop has a very complete set of Shortcut keys which are described here. near the end of the Help Documentation.

► What are some problems and solutions for importing DXF files?

When importing DXF files in from other CAD systems, such as AutoCAD, TurboCAD, Rhino, etc., the files will be opened in the original size and position.

Problem: Vectors did not import correctly

DXF files from other CAD systems may often appear as individual lines and arcs after being imported and cannot be V-carved or pocketed between unless the vectors are joined together using the tools supplied within Vectric Products.
These lines can be profile machined using a Profile-On toolpath, but the individual vectors will machine separately which may result in very jerky machine movements and slow machining times.

Solution: Join the Open Vectors

Use the Join Open Vectors tool to join the lines and arcs together so they can be machined more efficiently. The Join Open Vectors tool can be found within the Edit Objects section of the Drawing Tab in Cut2D, VCarvePro and Aspire.
In addition, Aspire and VCarve Pro have the ability to convert vectors into all lines, all Bezier Curve or all Arcs using the Fit Curves to Vectors tool which can greatly improve cut quality on some machines.

Problem: DXF file fails to import

If a DXF file fails to import, it may be due to the DXF version or the DXF file contains entities that Vectric software does not support.

Solution: Export in another format

If this is the case, try exporting the file again from the original CAD system in AutoCAD R12 or R14 format as these tend to be more compatible. The ability to export in older versions is normally offered by all major CAD systems. If needed, please consult your CAD application documentation for full details on exporting vectors.

Problem: Imported Vectors do not contain original Bezier Curves

The DXF formet does not support Bezier Curves, and can only save Arc curves and Straight lines.

Solution: Export in another format

In your original application, use a different format to save your vectors, such as Ai or EPS. Alternatively, modify your design before saving to convert the Bezier curves to Lines and Arcs, which will export correctly in a DXF file.

► Special Characters - Draw Text

Windows has support for a multitude of characters not seen on the Keyboardsuch as: ¢, ¥, ½, ©, and ¿.

In Vectric software that has support for Drawing Text, you can use the Windows Character Map to copy and paste these special characters into the Text editor to use them in your designs.

You can also use the ALT+ combination to type these fonts, and the combinations for each character can be found in the Windows Character Map.

You must also have selected a font that has support for these special characters. If you select a font that does not have support for these characters they will appear as a blank box, or some other generic symbol. There are to many variations on the Windows fonts to list the supported types here.

► How do you determine which side of an open vector is the right or left?

Select the vector and press N, the short-cut key for Node Editing. The small green square at one end of the vector is called the Start Point. If you start at the Start Point and follow the vector toward the node at the other end, the right side is on the right, the left side on the left. It may also help to visualize walking along the vector from the green Start Point to the other end.

► How do I display all the Alignment icons on the Drawing Tab?

By default VCarve 7.0, Aspire 4.0 and higher will display a single icon to access the Alignment Tools Form. If you want to display more Alignment icons on the Drawing Tab you can check the option at the bottom of the Alignment Icons form:

Checking this will add a section of icons to the Drawing Tab containing the major alignment options. If you have limited screen area you can uncheck this option to return to the default behavior.

---

► How can I work with a drawing that has both metric and imperial measurements?

First, setup your project for the units you want (inches or mm). Then, when you are provided a measurement using the other units, you can use the program's ability to evaluate mathematical expressions in the data input boxes to quickly convert the measurement to the needed units.

• To input a measurement given in inches to its metric equivalent, you would enter the inch value in the data input box, followed by *m=. For example, to enter 3 inches in mm, in the data input box you would type 3*m=. As soon as you press the = key, the input value will change to the metric equivalent of 76.2 mm.
• To input a measurement given in mm to its imperial equivalent, enter the mm value in the data input box followed by *i=. For example, to enter 130 mm in inches you would type 130*i= in the data input box, again without the quotes. As soon as the = key is pressed, the input value will change to the imperial equivalent of 5.1181 inches.

► How can I import the image if my PDF does not contain vector information?

PDF files can contain vector information, bitmap information or a combination of both. If you cannot successfully import a PDF file and get a message that it only contains bitmap data, your only option is to convert it to an image format the program can import using one of the following methods:

• The quickest and easiest way is to open the image in a viewer (depending on your PC, double clicking on the file name will normally open the image in an installed program), then use Print Screen or some other type of screen capture program to capture the image and save in a format that can be imported.
• You may have another program installed on your PC that will open the PDF image and allow you to export or Save As in a format that can be imported successfully.

► How can I close an open vector?

If you have multiple open vectors you want to close, the easiest approach is to use the Join Open Vectors tool. This very powerful tool will show you how many open vectors are currently selected and how many will be closed using the current Tolerance setting once you select Join.

Note: Your design may have open vectors as part of it's design, such as lines. Keep this in mind as you work to join only the open vectors that need to be joined.

The Tolerance setting determines how close two vector ends must be for the Join open vectors tool to be able to join them. Sometimes you need to increase the Tolerance setting until they will all close, but be careful with larger values as vectors may join incorrectly. Be sure to check the vectors carefully after you select Join to verify the results. If the results are not what you want, select Edit Menu ► Undo to reverse the operation and enter a smaller Tolerance value. Try to join as many as you can properly do with this tool, then use the next technique to join the remaining ones.

If you only have one vector to join, or a unique situation such as a very large gap, these three additional Join Tools may be a better approach. The tool names describe how the tool will fill the gap between the vector ends.

• Close vectors with a straight line
• Close vectors with a smooth curve
• Close vectors by moving end points to a common point

► How can I change the Start Point of a vector?

Select the vector and press N, the short-cut key for Node Editing.

If a node already exists where you want the Start Point to be, you can either hover the mouse pointer over it, right-click to open the Node Editing menu ► Make Start Point or hover the mouse pointer over the node and press P, the short-cut key to Make Start Point.

If a node doesn't exist where you want the Start Point to be, hover the point of the mouse cursor over the spot you want the Start Point to be and press the short-cut key P. This will create a new node at that spot and make it the Start Point, all in one operation.

Note: The Start Point must be at one end of an open vector but can be anywhere on a closed vector.

► How can I change text spacing (kerning)?

The The Edit Text Spacing and Curve tool found in the Drawing Tab allows precise adjustment of text.

► How can I add more fonts?

Additional True Type and Open Type fonts (.TTF) can be obtained from many sources and available to use once the font has been properly installed the Windows Font Directory and the program restarted.

This is not hard to do and typically if you right click on the font file, it will give you the option to install the font. If that option is not available, the exact process can be found in the Help Document for your version of Windows.

The included Single Line Fonts are installed during the program's installation and cannot be changed or added to.

► Do I need to use layers?

No, you do not need to use Layers, but understanding and learning how to work with them can dramatically increase productivity and make complex jobs much easier to organize and work with.

Some examples where Layers can help you:

• You can organize Layers by the toolpath that will be used, such as drilling, pocket, V-carve and cutout. Used in conjunction with Toolpath Templates and this becomes a very powerful production tool.
• A different color can be assigned to each Layer, helping to visually organize a complex project in the 2D Design window.
• Layers can be made visible or invisible, allowing a complex project to be worked on one portion at a time.
• Layers provide a quick way to create backup copies. Select the vector(s) you want to backup, right-click and select Copy to Layer. Create a new Layer, call it Backup or similar, and uncheck the box to make it invisible.
• When you import a bitmap or vectors from another source, a special layer will be automatically created for this. After performing the operations you need, those layers can be deleted or made invisible.

► Can Vectric software run plasma/water jet machine tools?

Vectric software is designed specifically to be used with 3-Axis CNC machines and has not been optimized for use with a Plasma or Water Jet machine, however some users have successfully used it to operate this type of equipment.

Aspire 4.0, VCarve 7.0 and higher include an option to add plasma loops onto acute corners of toolpaths.

We would recommend looking closely at the options available in the Trial Version of each program before specifically purchasing them for use with these types of machines. Another good source of information on how the software has been used sccessfully is to search the Main Forum.

► Can I work with an image file (bmp, tiff, jpeg etc.)?

You can import the following file types into Aspire, VCarve, Cut2D (Pro/Desktop):

File Suffix	Format summary
BMP	Windows Bitmap Format
JPG, JPEG	Compressed format commonly used for digital photographs and websites
GIF	A common web format, usually with a limited number of colors
TIF, TIFF	A compressed format, including a 16-bit version
PNG	More recent format with a good range of properties

Once imported, you can use the Trace Bitmap tool to automatically trace the image or you can manually trace the image using the drawing tools.

► Can I use a Snap Grid or Guide Lines to help me work with vectors?

Yes, Snap Grid and Guide Lines can be very helpful when designing new projects.

Use Edit ► Snap Options or the short-cut key F4 to open the Snap Options form and select the features you want.

You can find detailed information on each option setting in the Help Contents or Reference Manual.

► Are there any shortcuts for controlling the view in the 2D Design window?

Yes, there are View Control shortcuts available to help with adjusting the view in the 2D Design window.

SketchUp

► What is SketchUp?

SketchUp is a free 3D modelling application from Google. It allows you to create accurate diagrams of your designs in a true 3D environment.

To learn more about SketchUp visit here. http://www.sketchup.com

► Why is my imported model much too big or much too small?

Check that you are using the same scale in both Aspire and Sketchup. If you use mm in one and Inch in another, this can cause confusion when you are importing to Aspire.

The only time you can change the measurements for Sketchup is to change the Template option when first opening the software.

► When I import my model, I get multiple copies of components.

When importing a model for vectors, any component attached to multiple layers will be imported multiple times.

To stop this select Only import visible data on selected layers and deselect all layers except for one instance of each component.

► When I import a flat panel with a rounded edge as a vector import it does not record the rounded edge.

2D vectors cannot record something from a 3D image, either use the 3D component import function, or approximate the desired curvature of your edge using a Profile tool path combined with a Roundover Toolbit.

As long as your material and toolbit settings are accurate to your equipment, the Toolpath Preview will accurately show you the final effect as long as there is no requirement for an undercut.

Undercuts cannot be viewed in Aspire or VCarve Pro.

► What version of Aspire or VCarve should I use to open SketchUp files?

You should use Aspire 4.514 and higher or VCarve Pro 7.514 and higher to open SketchUp files.

Always check for the latest updates using the Help Menu ► Check for Updates

Aspire 4.514 and VCarve Pro 7.514 can open Sketchup 2014 files and older.

Aspire 8.5, VCarve 8.5 and Cut2D 8.5 can open Sketchup 2016 files and older. (Vectors only for Cut2D).

► What sort of designs should I be using SketchUp for with Aspire and VCarve?

Sketchup and the Aspire/VCarve Pro Vector importer is designed to allow you to work smoothly with flat panel designs, which will allow you to visualise the final product before having the components pulled apart and made ready for cutting.

This will turn a 3D models edges into vector lines ready for you to assign toolpaths to.

Certain design aspects need to be considered in your Sketchup design to allow for easy importing, such as component naming and Layer ordering.

► What should I save my Sketchup model to import Vectors to Aspire or VCarve?

Aspire V4.514 and higher and VCarve V7.514 and higher can read Native Sketchup format (.SKP).

Load them from File Menu ► Import... ► Import Vectors...

Also you can now drag and drop .SKP files directly from a Windows folder into the 2D Drawing window to begin the Vector import process.

► What does Auto Orientate do in the Vector Import dialogue for SketchUp?

As most components want to be cut so that the largest face is face up on the CNC Router, if this option is selected, all the components in your Sketchup file will be rotated so that the face facing up is the largest.

If your design requires thin pieces that have a thicker profile then face, this option may not be suitable. Position your components within Sketchup with the correct orientation for cutting before importing.

If you are finding that your top face is not being used as the top face by the Sketchup Importer, (due to having a smaller surface area then the bottom face) then you can force it to stay the right way up by adding a colour to the top face in Sketchup.

Then when you are importing the vectors into Aspire/VCarve you can change the Orientation option to Orientate by Material and pick your colour from the dropdown menu. This will inform the importer exactly which way up you need the model be.

► My model does not look as smooth as it did in my other 3D package.

Most 3D packages apply a visual smoothing that makes a 3D model appear to be smoother than it really is.

Aspire will only show a 3D model as it really is, with no smoothing applied. This is to ensure that the on screen representation correctly resembles the final cut piece.

Once your 3D model is in Aspire, you can use the Smooth Components tool to take some of the edges off your model, but it is more effective to increase the polygon count within your 3D package and reimport it.

► My 3D SketchUp model is not importing to flat panels correctly in Aspire or VCarve

To recognise the models parts as possible panels to create vectors from, a Sketchup model needs to be modelled as individual components, rather than the entire design constructed as one piece.

Break the design apart into its individual component parts within SketchUp and reimport it.

► I have updated Sketchup and now cannot open my files in Aspire or VCarve

With the updates to Sketchup, their files have become version locked.

This means that our software can only open particular editions of Sketchup files.

Aspire V4.514 and VCarve Pro V7.514: Sketchup 2014 and earlier.

Aspire v8.024 and VCarve Pro/Desktop V8.024: Sketchup 2015 and earlier.

Aspire v8.5, VCarve and Cut2D Pro/Desktop V8.5: Sketchup 2016 and earlier. (Vectors only for Cut2D)

If you have a later version of Sketchup, then when saving a Sketchup file, you will need to change the Save as Type to an earlier version of Sketchup.

Saving a SKP fie this way will allow you to then import it into your Aspire and VCarve Pro/Desktop software.

► Why I can see through my model when it is imported?

Your model has a hole in it from when it was saved in Sketchup, reopen it in Sketchup and use the drawing tools to cover the hole.

Check the face orientaion to make sure the model is not inside out.

► How do I import SketchUp models?

For Aspire 4.514 3D components: Once you have a new project opened, or an existing project opened, use the File Menu ► Import ► Import Component/3D Model.

There are additional options to import and for more detail on this visit Aspire 4 Tutorial F03 Click here for Aspire Tutorials.

For VCarve Pro 7.514 and Aspire 4.514 Vectors: Once you have a new project opened, or an existing project opened, use the File Menu ► Import ► Import Vectors...

This will allow you to select your desired .SKP file and load the Sketchup File Import window.

From here you have various options to modify how the 3D Model is turned into 2D Vector lines that can be used in the software.

You can also use the Windows Drag and Drop to drop a .SKP file directly onto an opened projects 2D View which will begin the import process.

► How can I import a 2-sided SketchUp model?

Sometimes you want to machine a model that does not easily fit onto a flat plain for CNC machining. This can be handled just like any other 3D model import.

See our existing Tutorials on 2 sided machining here.

► How can I get the best results with the SketchUp Vector import?

If possible, take your Sketchup design and lay out the components flat with the pieces orientated as if you were laying them out to cut. This will ensure that when they are imported, the vectors are exactly where you want them to be.

When working with layers it is important to ensure that all parts of the element you are working with exist on the correct layer.

Due to the nature of Sketchups layers system, it is easy to spread a model over multiple layers, which will make importing it more difficult.

For more detail, please read the Sketchup Importing Guide.

► Can I import SketchUp models into Aspire/VCarve?

Yes you can.

Aspire can now load 3D models from Sketchup, in the exact same way you can from .STL files.

This is applicable for Aspire 4.514 and higher.

VCarve and Aspire can both now import 2D Vectors from Sketchup files.

This is applicable for both VCarve 7.514 and Aspire 4.514 and higher.

Toolpaths

► How can I open a file from Cut3D (V3D), Vector Art 3D Machinist (V3M) or PhotoVCarve (PVC) in Aspire, VCarve or Cut2D?

Yes, Aspire, VCarve Pro/Desktop and Cut2D Pro/Desktophave the ability to import the toolpaths that have been created in Cut3D (.v3d), Vector Art's 3D Machinist (.v3m) and PhotoVCarve (.pvc).

Once imported, the toolpaths can be used as part of the design in larger projects.

Note: While Aspire is capable of almost all operations the other programs can perform, the ability to import toolpaths from these programs was included to provide flexibility between users.

Here is an overview on how you would do this:

• You first need to setup and create the toolpaths in Cut3D, 3D Machinist (limited to Vector Art 3D's .v3m file format) or PhotoVCarve and save the file.
• Then in Aspire, VCarve Pro or Cut2D you would use the command File Menu ► Import ► Import PhotoVCarve or Cut3D toolpaths.
• Once imported you can use the visible grayscale of the image and position it where you want for the project's design. The program will then automatically provide an offset to ensure that is where the toolpaths will machine in your project.

Click here to find a Tutorial on Importing 3D Toolpaths into Aspire or VCarve Pro

Click here to find a two part Tutorial on Importing a 3D project into Cut2D

Note: Some tutorial material is written for Vector Art 3D's free 3D Machinist program. The steps for Cut3D would be identical.

See Also:
• VCarve Pro 6 & Aspire 3 Tutorials

► How can I tell how deep my V-Carving is?

After the software has calculated a toolpath, it displays a summary of the toolpath data on the 'background' of the Toolpath tab. This is only visible when no other form is open on the Toolpath tab, so you may have to close the Preview form to see it.

As you click on different toolpaths names in the Toolpath List this information will be updated for the highlighted Toolpath. Find the Min. Z line and it will tell you the deepest that toolpath will cut.

As well as showing the Min. Z value for the selected toolpath, this information also includes feed rates, tool information and estimated machining time.

► Will my CNC do V-carving work?

Most modern CNC machines will certainly be able to cut 3D V-Carved projects. If your machine can move the X, Y & Z axes simultaneously (all at the same time), then it should be capable of V-Carving.

You can confirm that the software is compatible with your CNC machine by downloading the Trial Versions, opening the included sample projects and saving the toolpaths with the correct post processor for your CNC machine. Then you can actually cut samples at your machine and confirm it will work with the software.

If you have any additional questions, please contact us at This email address is being protected from spambots. You need JavaScript enabled to view it.

Click here to open the Trial Software webpage

► Why is the machined edge of my dish model rough or have a ridge around it?

Anytime you create a project with a dish or other recessed shape it is good practice to create a Zero Plane for the shape to merge with. This allows the software to better define the exact point where the recessed shape meets the surface, which will result in a better toolpath and smooth machined surface.

A ridge around the recessed shape could be caused by many reasons and they are typically associated with how the project has been designed and set up.

We cannot cover all the possibilities here, but one quick check you can make is to check is the Model Position in Material. Open the Material Setup form using the icon on the Toolpath Tab and verify the Gap Above Model is set to 0.0.

If this does not help, it is suggested you create a new post on the main forum and ask for possible ideas and solutions. Providing the file (only if it does not contain any protected 3D models or vector designs) always helps, as does pictures and screen prints. Normally, the more information you can provide the faster and better the responses will be.

► Why is no toolpath being calculated for the vectors I have selected?

There could be a few issues that would cause this and most should generate a Warning or Error message.

Some quick things to check include:

• Tool too large to fit in the area. Try increasing the size of the area slightly or Edit the tool and very slightly reduce the bit diameter just for that toolpath. For example, if you are trying to cut a pocket 0.25 inch (6mm) wide with a 0.25 inch (6mm) end mill you can adjust the pocket width or 0.251 inch (6.02mm) or edit to tool's diameter to 0.249 inch (5.98mm).
• Use node editing to check the vector(s) for small loops or overlapping segments. This is a very common problem when the vectors have been exported from another program.

If nothing is apparent, this type of problem is always good to post on the main forum and if the file does not contain any protected images or models, posting the file helps considerably. As a minimum, including some pictures and screen prints will help other forum members offer suggestions and ideas.

► Why does my actual cut part not look like the Preview Image?

The more you use our programs, the more you will appreciate the accuracy of the Toolpath Preview and how it can help achieve superior results at your machine.

However, there are issues beyond the program's control that can result in your machined project not looking like the Preview image.

There could be many reasons for this, but here are a few to consider and check:

• Do not setup a toolpath that exceeds the cutting length for the bit you will use.

• Be sure you set Z Zero at your machine to the same point (Top of Material or Top of Machine Bed) that was set in the program when the toolpaths were calculated.

• Be sure you set the X,Y Origin to the same relative position at your machine that was set in the program when the toolpaths were calculated.

• Be sure you have installed the same bit at your machine as the toolpath was calculated for.

• For V-carving, it is very important to use the exact same angle V-bit as the toolpath was calculated for. A different angled V-bit may have been installed at the machine OR the actual angle is slightly different that what the bit manufacturer marketed it under. A forum member, Paul Z, has developed a quick and easy way to find out exactly what angle your V-bit is without the need for expensive measuring equipment. Click here to see Paul Z's guide.

• Verify the actual Material Thickness matches the Material Thickness set for the project.

• Double-check all the Tool Database setting for the bit you are using. Sometimes it is easy to create or copy a tool and input the wrong diameter.

• Verify the Feed Rate and Plunge Rate settings are correct for your machine and material, and have the units you want.

If none of this helps, you can post your information on the forum to get other's ideas and suggestion or contact This email address is being protected from spambots. You need JavaScript enabled to view it. for assistance.

► When should I use a Start Depth?

You would typically use a Start Depth when setting up a toolpath that will cut where material has already been removed by another toolpath. When applied properly, this can result in significant time savings when machining some projects.

A good example would be where a Pocket toolpath has already removed 6 mm of material and you want to cut text at the bottom of the pocket that will be 3 mm deep. In this case, you would set the Start Depth to 6 mm and the depth you want the text to be cut, 3 mm, in the Cut Depth.

Note: When you have used Start Depth in a toolpath, always be sure to run the toolpaths in the correct order. For example, running the Text toolpath before the Pocket toolpath in the above example could result in bit breakage or poor results as the Text toolpath is now removing 9 mm but with the same setup that was intended to only remove 3mm of material.

► What is the difference between changing a tool's settings in the Tool Database and Editing a tool in the Toolpath setup?

When you change a tool's setting in the Tool Database, it changes the default settings for that tool and these are the settings that would appear the next time that tool is selected for a toolpath.

After selecting a tool for a toolpath, you have the option to Edit that tool and make changes to the default settings that will apply only to that toolpath.

► What is the "Solid" option?

The Solid Option is now a toolbar button: Toggle toolpath 2D drawing style (Wireframe or Solid)

An easy way to visually check you have correctly set up a 2D toolpath is to use the Solid option available on the Toolpath Tab.

First, make the toolpath visible by checking the box left of the toolpath's name, then check the box under the Toolpath List labeled Solid. This will place a solid blue line in the 2D window that represents the exact cut path and width of the selected bit and you can quickly see if the toolpath is cutting where you expect it to.

Tip: This is a very good way to visually see if the selected bit can fit into all the areas you want, such as profiling around text. If it does not, you can recalculate the toolpath using smaller diameter bits until you find the size that will work or make changes in the design.

► What do I need to reset after a tool change?

Once you have set the material up on your machine you need to set X,Y Origin in the same location in reference to the jobs position on your CNC as shown in the project's Material Setup. Once this is done, it is important that this is not changed or reset during the job because all the different toolpaths will reference from this point.

However, setting Z Zero accurately following each bit change is important to ensure accurate cut depths by each tool. Be sure to set Z Zero to either the Material Top or Machine Bed depending on how the project has been setup in the Material Setup.

Tip: It is a good practice to pick a spot and Z Zero every bit at that same spot during a project. Be sure to look ahead and don't pick a spot that may get machined away by one of the toolpaths.

► What controls the depth where the tabs are in a toolpath?

The bottom of tabs are always at the Cut Depth for the toolpath and extend upward by the Tab Thickness set during the tab setup.

If you set a Cut Depth deeper than the Material Thickness to intentionally cut past the bottom of the material, be sure the tab Thickness is enough to still appear in the material.

Also, when using a Start Depth other then 0.0 with tabs, if the Start Depth is below the top of the tabs, some or all of the tabs will be machined away.

► Saving Images with a plain background?

If you want to save an Image without any background color, which is a useful feature if the image is to be used in a brochure or other type of publication, follow these steps:

• * Select View ► Use Shaded Background to uncheck that feature
• * Save the image using the .PNG file format

► In the Profile Toolpath, what is Allowance Offset used for?

The Allowance Offset only applies to the Outside / Right and Inside / Left options. It provides a quick and easy way to calculate different size toolpaths using only one defining vector.

• For the Outside / Right option, a positive offset value will leave more material on the outside of a closed vector or to the right side of an open vector. Likewise, a negative offset value will remove more material from a closed vector or leave less material to the right side of an open vector.
• For the Inside / Left option, a positive offset value will leave more material on the inside of a closed vector or to the left side of an open vector. Likewise, a negative offset value will remove more material from the inside of a closed vector or leave less material from the left side of an open vector.

It is easy to visually check the toolpath in the 2D window to ensure the offset is doing what you expect by using the Solid preview option.

► In the Pocket Toolpath, what is Pocket Allowance used for?

The Pocket Allowance allows you to quickly create a toolpath that will machine the pocket either smaller or larger than the defining closed vector.

• A Pocket Allowance of 0.0 (the default) will create a pocket the exact size of the defining vector.
• A positive Pocket Allowance value will make the pocket smaller than the defining closed vector.
• A negative Pocket Allowance value will make the pocket larger than the defining closed vector.

It is easy to visually check the toolpath in the 2D window to ensure the offset is doing what you expect by using the Solid preview option. 

► How do Start Depth and Cut Depth work together?

When you set both a Start Depth and Cut Depth in a toolpath, the Cut Depth will begin at the Start Depth and add to it, so the total depth of cut will equal the Start Depth plus Cut Depth.

For example, setting Start Depth to 6 mm and Cut Depth to 3 mm will result in a total depth of cut of 9 mm.

► How do I use the two Safe Z settings, Z1 and Z2?

When you open the Material Setup form using the Setup button on the Toolpaths Tab, you will see settings for Clearance (Z1) and Plunge (Z2). These are also referred to as the Safe Z settings:

The Clearance (Z1) is the most important setting. 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.

The Plunge (Z2) is an added feature. As well as specifying a rapid clearance gap for rapid positioning moves above the work piece, 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 (Z2) gap to a smaller value than the Clearance (Z1) 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 (Z1) gap has to be specified to avoid clamps etc, this feature can save a considerable amount of machining time if there are many plunge moves in the job.
• Setting a value of 0.0 for the plunge gap will also disable this feature.

Note: Not all machines can take advantage of this feature.

► How do I transfer the toolpaths to the machine tool?

There are exceptions, but the vast majority of users copy their toolpaths to some type of flash drive and take this to their machine or save over a network connection to transfer the post processed toolpaths directly to their machine's controller.

If that does not work with your machine, you should contact the machine's manufacturer or distributor to find out the required procedure.

► How do I stop the toolpath cutting past the edge of my 3D model?

Aspire and VCarve V8.0 and Higher:

A new feature of Aspire and VCarve, is the option to automatically limit a 3D toolpath to the model boundary.

Just select this option when setting up your 3D toolpathing.

Aspire v4.5 and Lower:

If you select a closed vector shape before calculating the 3D Roughing and 3D Finish toolpaths, the toolpaths will observe the vector as a machining boundary and stay inside of it. Without this, the toolpaths will calculate for the entire surface of the material which can add significantly to the machining time.

There are a couple of ways to create this machining boundary vector. It may be as easy as creating a vector shape with the drawing tools (circle, ellipse, rectangle, etc.) or you may want a vector that follows the exact profile of the 3D model. In this case, you can use the Create Vector Boundary From Selected Components tool found on the Modeling tab or use the Trace Bitmap tool found on the Drawing tab.

Once the boundary vector has been created, the 3D Roughing and Finishing toolpaths include a setting called Boundary Vector Offset, which can be adjusted to allow the toolpaths to extend past the boundary by the set amount or have them short of the boundary by the set amount.

► How do I setup the start point of the toolpath?

For the Profile Toolpaths you can use node editing to place the vector's Start Point where you want it.

In Aspire and VCarve Pro, be sure to check the box that says Use vector start points (don't optimize) when setting up the Profile Toolpath.

In Cut2D, the default action is to use the vector start points under most conditions and the user has no external control over it.

► How do I set the Cut Depth when V-carving?

The V-carved Toolpath is unique because there is no way to set the Cut Depth. The toolpath requires a closed vector shape and will move the V-bit as deep as required to machine to the two vectors on either side of the bit.

In general:

• The wider the gap between the two vectors, the deeper the V-bit will cut.
• The narrower the gap between the two vectors, the shallower the V-bit will cut.
• The higher the included angle of the V-bit, the more 'pointed' it is and the deeper it will cut.
• The lower the included angle of the V-bit, the 'flatter' it is and will cut shallower

Note: As long as you have the Material Thickness accurately set in the Material Setup, the program will warn you if the depth of the V-carving will be deeper than the material thickness.

► How do I machine a single line font?

The Single Line Fonts included with the program are designed for drag type engraving tools using the Quick Engraving Toolpath.

However, you can machine them with ordinary router bits (typically V-bits or engraving bits) using the Profile Toolpath with the On option selected and a shallow Cut Depth set.

The Toolpath Preview will allow you to try different combination of bits and Cut Depths until you get the look you need.

► How do I ensure my bit will not hit a clamp when traveling across the machine bed?

When you open the Material Setup form using the Setup button on the Toolpaths Tab, you will see settings for Clearance (Z1) and Plunge (Z2). These are also referred to as the Safe Z settings:

Clearance (Z1), which is also referred to as the Safe Z is the height above your Z Zero reference point that the bottom of the bit will rapid at across the machine bed.

If you are using clamps or have another need for the bit to travel above a certain height, this value is what you will set to control that.

► How can I remember what Allowance Offset or Pocket Allowance will change in my toolpath?

When you enter a positive value for either offset, it will always offset the cut line to leave extra material that would later be removed with a separate finish toolpath.

If you enter a negative value for either offset, it will remove more material than the defining vector would normally allow.

► How can I make copies of a toolpath to cut multiple versions of the same part?

Once you have setup a toolpath on one of the parts, double click on the toolpath name to open it for editing. Then select all the identical parts you want to toolpath and recalculate the toolpath.

Additionally, some control systems allow a single toolpath to be cut multiple times. This is totally a function of the control system and you would need to contact your machine's manufacturer or control system's developer for specific information.

► How can I machine a project which is larger than my CNC work area?

The Tile Toolpaths tool will break the entire project's toolpaths into smaller tiles that can be machined one at a time.

You have a choice of how you can break up the toolpaths which will probably be driven by your machine's size and the current project. The choices are to create individual tiles using separate pieces of material, which are later assembled to form the complete project or using one long piece of material you can reposition and machine it in sections.

You can find more detailed information in the Help Contents and view a tutorial video on the process in the Training Materials section.

Click here to open the Tutorial page with the Tile Toolpaths video

► How can I improve the edge quality of my 3D model when machining it?

It can sometimes be very challenging to obtain good vertical edges with 3D toolpaths.

If a vertical edge is part of the 3D design, there may not be much that you can do unless the model can modified and the design allows a vertical edge to be replaced with a slightly angled edge.

However, if the vertical edge is the outer edge of a design and will later be cut with a Profile type cutout toolpath, a good approach is to use some technique to limit the 3D toolpaths from cutting this vertical edge.

There are many ways to do this and the best approach many times depends on the shape of the 3D components. Some suggestions are:

• Use a boundary vector and set the Boundary Vector Offset to keep the 3D toolpaths on the top surface of the 3D model.
• Create a 3D component the same height (or close to it) as the edge you are trying to protect but larger in size and merge it with your project. Then use a boundary vector and Boundary Vector Offset that allows the 3D toolpaths to flow off the model and onto this new model a short distance. Finally, use a Profile toolpath (with normal tabs if required) to cut the vertical edges.
• Aspire Only: If the design was created with a Two Rail Sweep such as a molding, modify the Two Rail Sweep  to add either a flat surface or angled edge (typically called a draft angle). Calculate the 3D toolpaths using the new wider vectors but cut it out using the original vectors with a Profile toolpath (with normal tabs if required).

► How can I improve the cut quality when working with difficult materials and/or deep V-carvings?

When cutting hard materials or very deep v-carvings the tool may vibrate or chatter causing marks on the job.

A tip for improving the surface finish is to:

1. Calculate the toolpath using multiple Z Level passes
2. On your machine - Set the Z Zero position for the tool slightly high (i.e. 0.02 inches or 0.5mm) and run toolpath 1. (this will leave material on the job)
3. Calculate a second toolpath that cuts the job in a single pass (Be sure to set Pass Depth greater than the actual Min Z depth displayed for toolpath 1
4. On the machine - Set the Z Zero position correctly and run toolpath 2. This toolpath will remove the remaining 0.02 inches / 0.5mm cleaning-up the surface finish.

► How can I get an estimate of how long the toolpath will take to actually cut?

You will find Estimated Machining Times associated with toolpaths found in different places depending on the program and the summary list below should help.

For all the programs, you have to take some steps to make this estimate as accurate as possible for your machine:

• First, set the Rapid Rate to the correct value and units for your machine. For most machines, this is set in the software that controls the machine.
• Then, actually time some toolpaths at your machine and adjust the Scale Factor for those toolpaths until the Estimated time for that toolpath is close to the actual time you measured.
• After you do this a few times, the best Scale Factor for your machine should become clearer.

Note: This is only an estimate and does not include any adjustments the machine's control system may make such as Acceleration/Deceleration settings. As such, it is hard to find one scale factor that will work with all the types of toolpaths. However, it should get you close and help with quotes and machining decisions.

Where to find the Estimated Machining Times:

• Cut3D: At the bottom of the Roughing, Finishing and Cutout Toolpath Setup pages and on the Preview Machining page where you can adjust the Rapid Rate and Scale Factor.
• PhotoVCarve: On the Preview & Save Toolpath page.
• Aspire and VCarve Pro: Click on the Toolpaths Summary icon on the Toolpath Tab that will open a summary sheet showing the individual times for all the calculated toolpaths and a Total Machining Time. You can hover the mouse over the name of the Toolpath in the Toolpath List and the tool-tip will pop up with information about that toolpath including the Estimated Time.

► How can I find the correct post processor for my machine tool?

After you click the Save Toolpath icon, there is a pull-down list with all the post processors currently stored in the PostP folder (in the Application Data Folder) on your computer. Scroll down this list, find and select the correct post processor for your machine.

You only need to do this once. The next time you open the Save Toolpath form the last post processor selected should show as the default post processor.

If you are not sure of the correct post processor for your machine, you can contact the machine's manufacturer or distributor, ask on the manufacturer's forum, ask on the Vectric Forum, or contact Vectric at . This email address is being protected from spambots. You need JavaScript enabled to view it.

► How can I create a new custom tool?

If you need to create a new tool that is not one of the standard types, you would create it as a Form Tool. With this feature you can match any router bit that does not have an undercut, such as dovetail bits and Keyhole bits.

You can find a detailed description in the Help Contents / Reference Manual and a How-To article at the link below.

Click here for a step-by-step procedure.

► How can I control how many passes (depths of cut) my toolpath will take?

In most toolpaths you can set a Pass Depth for the selected bit. The program will create enough passes until it gets to the Cut Depth set for that toolpath.

In Aspire and VCarve Pro the 2D Profile Toolpath can be modified using the Edit Passes button which opens the Specify Pass Depths form.

Tip: The ability to Edit Passes and quickly assign different pass depths is a quick way to leave an onion skin to be removed by a final pass. It also provides a quick way to adjust Profile toolpaths using bits such as v-bits and ball nose bits where the amount of material removed would increase with each pass if a constant Pass Depth was set.

► How can I adjust the depth of my V-carving when it is too deep or too shallow?

If your v-carving is cutting too deep you have a few options:

• The easiest solution is the use the Flat Depth option near the top of the V-Carve / Engraving Toolpath form. This will still cut angled sides using a v-bit but the bottom will be flat and limited to the Flat Depth amount. This can be visibly different than a design carved to full depth without a flat bottom, but may be your only option especially if you need to work with the v-bits you have on hand.
• Use a v-bit with a larger included angle, which cuts a shallower v-groove. For example, a 90-degree v-bit will cut shallower than a 60-degree v-bit, and a 120-degree v-bit will cut shallower than a 90-degree v-bit.
• Reduce the size of the vectors to reduce the gap. Typically not practical once the design is set, but may be one option if you have a limited number of different angle v-bits available.

If your v-carving is cutting too shallow switch to a v-bit with a higher included angle (more pointed).

Tip: Sometimes you may find the best angled v-bit for your project is one you don't have. Find out what v-bits are commercially available in your area and create tools for them in your tool database. Then use them with the Toolpath Preview until you get the results you want. Now you know exactly which v-bit you need to purchase to complete the project. 

► Does Vectric software support Tool Changers?

Cut2D and PhotoVCarve do not support tool changers.

Cut3D, VCarve Pro and Aspire all support Tool Changers assuming you have the correct post processor selected (the Post-processor name should end with ATC for Automatic Tool Change).

You can confirm this for your CNC machine by downloading the Trial Versions, opening the included sample projects and saving the toolpaths with the correct Tool Changer post processor for your machine. Then you can cut samples at your machine and confirm correct tool changer operation.

Each toolpath must have had its Tool Number set in the Tool Database (edit the toolpath and click the Edit button).

The Tool Number is displayed in square brackets: [1]

Click Output all visible tool-paths to one file and all the visible toolpaths should be listed as shown:

---

► Can I create a tool with an undercut?

No, the Form Tool will not allow a bit with an undercut to be modeled since toolpaths using bits with undercuts cannot be previewed.

If you need to use a bit with undercut in a project, you can create a toolpath using a standard bit but run that at your machine with the undercut bit installed.

For example, you want to create a T-slot using a T-slot bit. You can create a toolpath using an end mill and preview that, realizing at your machine there will be a horizontal slot cut at the bottom of the toolpath. To do this safely and successfully, you need to have a good understanding of toolpaths, how to set up a single pass toolpath and possibly the use of Lead-ins and Lead-outs.

If you need help setting up a particular toolpath, asking on the Vectric Forum should get you the help you need.

► Can I control the speed of the Toolpath Preview?

Several settings can change the simulation speed when you preview a toolpath and the actual results will depend on your particular computer.

• Before previewing the toolpath, check or uncheck the 'Animate Preview' check box in the Preview Toolpaths menu. Having this checked will slow the preview down, having it unchecked will allow it to speed up.
• Changing the Preview Quality can make a difference on the amount of time it takes to generate the toolpath and preview it. The lower quality setting will allow the toolpath preview to go faster, but the resulting screen appearance will suffer. The higher quality settings will allow the preview go slower, but result in better screen appearance. You can change the Preview Quality by using Toolpaths ► Preview Simulation Quality.
• Aspire and VCarvePro add an additional feature called Preview Controls located on the Toolpath Preview form. These Preview Controls provide full video-like playback control of your toolpath. You can use this mode to analyze the tool moves in detail, moving step-by-step or until a tool retract. To begin using Preview Control, click on either the Run, Single-Step or Run to Retract buttons, which are summarized below.
• Aspire 4.0 and VCarve Pro 7.0 also add an option of a Speed Control slider which can be adjusted to slow down the speed that the toolpath simulation is run at.

► Can I add different types of preview materials?

Although the standard list of job preview materials provides a reasonable selection of woods, stones and metals to choose from, you may have a project that requires a special material type. For example, a customer may require their work to be carved into a special wood that is not in the default list of materials.

The Job Preview material list can very easily be edited to include your own material types and selection names, allowing your work to be previewed and saved in the same materials that you are actually planning to rout or engrave.

► Are there any shortcuts for controlling the view in the 3D Preview window?

Yes, there are View Control shortcuts available to help with adjusting the view in the 3D Preview window listed in the 3D View Controls section.