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

Watch this video to see this in action:

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 Mopens the Move form in interactive mode.

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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

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

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

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

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

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).

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

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

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

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

The Tool Database is used to make cutter management and selection very quick and easy, and reduces the possibility of programming jobs with incorrect cut depths and speeds and feeds. It allows pre-defined tools and settings (speeds, feeds, stepover etc.) to be selected from a list for a given machine / material.

The Tool Database can be accessed from the Select... button through the various Toolpath forms. You can open the Toolpaths Tab button or through the Toolpaths menu.

Watch this video to see this in action:

This is a summary of the main entities and relationships in the database. More details on those will be given in the next sections.

1. Tool geometry entities (organised hierarchically in the tree).
2. List of Materials (Managed through the Material Management dialog).
3. List of Machines (Managed through the Machine Management dialog).
4. Cutting Data set for each tool geometry. This includes the Cutting Parameters, and Feeds & Speeds, and are defined per machine / material.

Tool Properties are divided into two categories,

1. Tool geometry: This is the physical properties of the tool such as the diameter, tip radius, etc...
2. Cutting data: These include the Cutting Parameters and Feeds & Speeds of the tool. These values are defined for a particular material / machine.

The Tool Tree is located on the left-hand side of the Tool Database. Click on items in the list to see or edit their properties using the Tool Info section of the database window.

You can drag items up and down the list to change their order or drag them inside / outside of groups.

Duplicate the selected tool geometry or group in the list. If you're copying a tool, it will be copied without its cutting parameters.

The cutting parameters can be subsequently be:

• Copied from the same tool, different material.
• Tool with identical geometry, any material.
• Created with default values.

A tool database file can be imported into the currently open tool database. You will have several options:

1. Import: This will simply import the given tools under the selected group (or as a top-level tool / group).
2. Merge: This will attempt to merge the incoming tool group hierarchy with the current one (without any regards for selection)
   1. Overwrite: When it's faced with two similarly nested tools that have the same tool geometry, the cutting data of the incoming tool will overwrite the current tool's cutting data for the active machine / material.
   2. Without overwriting: A new machine / material will be created to contain the cutting data of the incoming tools.

This will go to the Name Format dialog to edit the name template for this tool type.

The name displayed here is then a result of evaluating the template in the current context (active machine, material and the cutting data defined for those as well as the tool geometry).

The name of a tool group can be defined directly through this dialog.

Various cutters can be specified in the database. Changing the cutter tool type is equivalent to creating a new tool, so all existing data for that tool (if any) may not be applicable anymore.

V-Bit

Engraving

Tapered Ball Nose

Ball Nose

End Mill

Radiused End Mill

Form Cutters

Diamond Drag

Drills

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.

To enter a link into the Note, go to the appropriate page in your Web Browser and select the URL of the page from the Address Bar.

CRTL+C to copy it and then in the Note Field, right click and use the "Paste" option to enter it into the Notes.

To use the HTML Link in the Note Window, hold the CRTL Key and click the link. This will open your computers default Web Browser and load the web page.

The cutting data is defined per material per machine. If the data is not defined already for a tool, we create it in a number of ways,

1. Create with some default values which you can then change for your purposes.
2. Copy from the same tool from a different material: This could be a sensible starting point if the materials have similar / close hardness.
3. Copy from a different (identical) tool from the same (or different material)

The maximum depth of cut the tool can cut. The Pass Depth controls the number of z level passes that are calculated for a toolpath.

For example, creating a pocket 1 inch (25.4 mm) deep using a tool that has a Pass Depth of 0.25 inches (6.35 mm) will result in the toolpath making 4 passes.

This value can be defined per machine / material depending on the machine's rigidity and the material's hardness.

The distance the cutter moves over when doing area clearance cutting. For example, when raster machining the cutter will machine along the X axis, stepover in the Y direction and return parallel to the first line of cut. The greater the stepover the faster the job will be machined, but this must be balanced with the material being cut and the tooling being used, to ensure that the tool does not break. Therefore, this property (along with all other Cutting Parameters can be defined per material / machine).

When stepover's greater than 50% of the cutter / tip diameter are used the software automatically adds 'Tail' moves in the corner regions of toolpaths to ensure material is not left on the job for offset based strategies.

When using V-Bit Tools, the Stepover fields automatically change to use the following options.

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.

This is the maximum speed at which the tool, when at 100% power, will still burn the material. This value is used for simulation purposes only. It should be calibrated to match your laser and material. A larger value will result in the simulated toolpath appearing darker.

You will need access to the Laser Module to create and simulate laser toolpaths.

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.

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

Before opening the tool database, draw to exact scale the Right side of the cutter geometry in the 2D Window Use the Node Editing tools to create the arcs and curves etc.

Select the vector, then open the Tool Database dialog and create a new tool. Then, set its type to Form Tool.

The selected geometry will be imported and a profile displayed in the window. Give the Cutter a meaningful name. Enter the cutting parameters - speeds and feeds etc for the various materials you've got defined.

Click the Apply / OK button to save the new cutter into the database list so it can be used at any time.

The Laser Module is a paid add-on for VCarve Pro which adds the following additional functionality:

• The ability to create Laser Cut and Fill Toolpaths
• The ability to create Laser Picture Toolpaths
• The ability to simulate a Laser Toolpath

If you have a licence code for the laser module then it can be installed by using the Help > Enter Licence Code menu item. Enter the licence code into the Licence Code field. The Licensed To field does not need to be changed.

You will have to restart you software to enable the features.

Laser Cut - Fill Toolpath is used for cutting out shapes or marking areas.

Cut-outs can take into account the kerf, or width, of the laser beam to maintain the precise internal or external size the selected vector shapes. Shapes can also be filled with stripes or hatching to create simple shading effects.

Like all other toolpaths the laser toolpaths can be simulated. However, in the case of laser toolpaths, the simulation does not remove any material but instead marks the surface of the current simulation model. This marking is meant to simulate the charring of the material when scorched by the laser.

Burn Rate 50

Burn Rate 100

Burn Rate 200

Due to the many combinations of laser, power, material and feed rate, it will be necessary to calibrate the simulation so that the simulation output matches the real-world results. This calibration can be done by modifying the Maximum Burn Rate property of a given tool. This is the maximum speed at which the tool, when at 100% power, will still burn the material. This means that a greater value will result in the simulated toolpath appearing darker. This value can be set in the Tool Database. We suggest you cut a sample file with the material and power settings that you would typically use and then adjust the Maximum Burn Rate so that the simulation matches your achieved results.

Introduction

The Laser Module enables both new tool types to represent lasers in the tool database, and also new laser specific strategies.

The laser module now provides independent records and variables for laser tools and toolpaths. Because these outputs have been separated from conventional router control, for most machines and controllers it is often possible to create a single Post Processor to work seamlessly with router or laser toolpaths, but please note that you may still need to ensure that the physical configuration of your machine is changed depending on the toolpath type.

There are generally 4 areas that need to be modified in a conventional Post Processor to extend it for Laser toolpath support.

• Add support for a new Power variable, which will be used by the new laser strategies.
• Add new laser-specific Post Processor Blocks to format laser toolpaths correctly for your machine and controller.
• Modify any existing Post Processor Blocks to ensure independent power and laser-specific behaviour.
• Add a flag to tell Vectric's software that this post now supports laser toolpath strategies.

The following sections deal with each area in turn and an example using the GRBL gcode controller is provided. These examples are from the grbl (mm & inch) post processor provided by default with Vectric's software.

Power Variable

Vectric's software will output the power setting for a laser toolpath in the range of 1-100%. We need to add a new variable to show how to format this setting for your particular controller. This is also the opportunity to scale the raw percentage value to the numerical range that your controller requires.

Example

For GRBL-based controllers, the power setting for a laser is typically aliased to the gcode spindle speed control command 'S'. In laser mode, the controller will respond to a spindle speed control change by adjusting the power of the laser instead. Although it can be set within the controller, the default setting for the maximum expected 'S' value - or laser power - is 1000.

For GRBL, therefore, we need to format the POWER variable to be a gcode 'S' command and scale its output value by a factor of ten so that it is in the range of 1 to 1000 (instead of the default 1-100).

The variable entry in the Post Processor reads:

VAR POWER = [P|C|S|1.0|10.0]

To break this entry down in plain English, we are saying that the POWER output from our toolpath should be used everywhere in our subsequent post definition file where we have the the variable [P]. But we should only only output a command as the POWER value changes (C). We will replace the [P] variable locations in our our toolpath output with the command 'S' (S). The power value should be formatted as a whole number with no decimal points (1.0) and should be multiplied from its default by a factor of 10.

New Laser Post Processor Blocks

To allow Laser control, there are new Post Processor Blocks available in the Post Processor. These are:

• JET_TOOL_ON - Output whenever the toolpath needs the laser on
• JET_TOOL_POWER - Output whenever the toolpath needs the laser power to change
• JET_TOOL_OFF - Output whenever the toolpath needs the laser off

Example

In our GRBL example we haved added the 3 new block types. For turning the laser on, GRBL makes use of gcode M4 command (normally intended for spindle direction, but 're-used' by GRBL for laser support ). We can now make use of our POWER variable, defined above as [P], to provide the required power value. The JET_TOOL_ON block is thus:

+---------------------------------------------------

+ Commands output when the jet is turned on

+---------------------------------------------------

begin JET_TOOL_ON

"M4[P]"

For turning the Laser off GRBL makes use of the gcode M5 command:

+---------------------------------------------------

+ Commands output when the jet is turned off

+---------------------------------------------------

begin JET_TOOL_OFF

"M5"

Finally for setting the power itself then for GRBL we just output the power:

+---------------------------------------------------

+ Commands output when the jet power is changed

+---------------------------------------------------

begin JET_TOOL_POWER

"[P]"

Modify Existing Blocks

We also want it to be the case that when we perform a feed move then we also output the power, so to do this we update the FEED_MOVE blocks to include [P].

We have to do that for all of the different feed move types.

In addition, we need to avoid plunge moves occurring when the laser is on. For conventional milling or routing, we need the spindle to be on before a plunge move, but for a laser it is crucial that we only turn it on after we have moved to the correct Z level (this problem manifests as 'overburn' at the beginning of each toolpath segement). To ensure that we can correctly separate these requirements, we may need to remove any spindle commands from plunge moves, or other block types (some may have them in the header, for example) and break these out into explicit SPINDLE_ON & PLUNGE_MOVE blocks. This will ensure that these moves are only made for non-laser toolpath strategies and in the correct sequence.

Example

For GRBL this is a simple addition to the end of the feed move statement:

+---------------------------------------------------

+ Commands output for feed rate moves

+---------------------------------------------------

begin FEED_MOVE

"G1[X][Y][Z][P]"

Remember that we set our POWER variable to only output on change (C) so note that in the output for feed moves at constant power, only an initial, changing, power command will be included. For some controllers, the number of commands that can be processed is a limiting factor on the speed of toolpath and for laser images, in particular, this can be mitigated somewhat by not sending uneccessary commands whenever possible.

For the separate GRBL spindle and plunge control the blocks are:

+---------------------------------------------------

+ Command output after the header to switch spindle on

+---------------------------------------------------

begin SPINDLE_ON

"[S]M3"

+---------------------------------------------------

+ Commands output for the plunge move

+---------------------------------------------------

begin PLUNGE_MOVE

"G1[X][Y][Z][F]"

You'll note that GRBL uses the M3 to control the router or mill. Also note that the plunge move requires the ability to move the machine in X & Y in order to support ramping.

Explicitly Mark the Post Processor as Laser Capable

Lastly a Post Processor will require the new Global File Statement LASER_SUPPORT="YES" added to be available for selection as a Laser Post Processor within the software.
This is only added to Post Processors for general use once the Post Processor has recieved complete testing by the creator.

Example

LASER_SUPPORT = "YES"

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

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

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

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

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

Exploded Flat Layout

Three Views - Front, Top, Side

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

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

Part Orientation

This section controls what Aspire 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 VCarve Procan be used to layout the parts with more control and across multiple sheets

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.

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, VCarve Pro 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.

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 VCarve Pro jobs. To allow control over what is imported you can choose to only import parts of the model which are on particular layers using this section of the dialog.

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

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

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, VCarve Pro will treat each SketchUp group / component as a single part UNLESS it contains other groups or components within it, in which case each lowest level group / component will be treated as a separate part.

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

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 VCarve Pro without the 'Replace outer boundary' option checked ✓. The part in the image has been ungrouped and the central vector selected.

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

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

This icon opens up the Moulding Toolpath Form. This form is used to create a toolpath from a drive

rail and a profile. The result of machining the toolpath is the extrusion of the selected cross-section profile along the pre-selected drive rail. Although strictly speaking the result of this is a 3D shape because it does not use a 3D model it is classified as a 2.5D Toolpath.

Watch this video to see this in action:

You now need to determine the toolpath position within the material. The Z Height of the toolpath is determined by the height of the selected cross section. You can interactively position the toolpath by pulling on the slider or you can enter exact values in the edit boxes.

From the 2D view, select the drive rails for the toolpath followed by the profile you wish to extrude.You may select multiple rails.The last selected vector is the Profile that you are extruding.

In the 2D view your rail vector will now be colored orange and will show a green square indicating the start point, along with arrows along the vector showing you the direction.

The direction and start point may not be what you intended, you can change the direction (and start point location on an open vector) by right clicking in the 2D View on the vector and choosing Reverse Rail.

The Clear Rail button on the form can be used at any time to empty your current selection; this will deselect the drive rail and if already selected the cross section too. This can be used if you want to change the selection without exiting the form.

After you have chosen your drive rail the next step is to select a cross section that will be swept around the drive rail to create the moulding. The cross section needs to be an open shape in order for this to work.

HoldCtrlTo select a cross section and click on the appropriate vector in 2D View and it will turn orange as with the drive rail, arrows and a green square will appear on it. In addition the drive rail will now have red lines shown on it. These indicate the side of the vector that the shape will be swept along. If this is not correct you will need to reverse the drive rail vector as documented in the previous section.

The arrows and green square on the cross section indicate the direction and the start point. The start point of the cross section will be attached to the start point of the drive rail. If you need to change the start point of the cross section you can do so by selecting the cross section with a right click and choose to Reverse Profile as shown in the image below. Doing this will change the arrow direction and move the green square and also change which end of the cross section is effectively hung on the drive rail when the toolpath is created.

The next step in this form is to select a tool to finish-cut the moulding shape. This would typically be a ball-nose or tapered ball-nose tool but that may vary depending on the shape you plan to cut. To select a tool use the Select... button to access the Tool Data Base. If the tool you require is already shown as the selected tool, you can use the Edit option to check and/or modify the tool settings for this particular toolpath.

Typically the Stepover value specifies the horizontal distance that the tool will step over and this is projected onto the 3D model. Checking ✓ the Vary Step Over option will instead adjust the step over based on the shape of the cross section profile vector rather than just projecting the standard pattern down Z. In cases where there are steeply curved, angled or near vertical edges this should result in passes that are closer together, in most situations this will improve the finish quality but also potentially increase the machining time

This choice will only become available when the option is checked ✓ to Machine Flat Regions when using the Larger Area Clearance Tool in the next section of the form. When this is active the software will look to identify flat areas of the cross section profile that can be machined with the larger tool. If these regions are detected and Skip Flat Regionsis also checked ✓ then the finish tool will avoid re-machining those flat areas as in most cases they should already have been completely finished by the Larger Area Clearance Toolpath.

If this option is selected, then two tools are used to cut the shape. In effect the Larger Area Clearance Tool is similar to a 3D Z Level Roughing toolpath and would be cut first. It will use the tool parameters to generate multiple depth 2D pockets following the direction of the selected rail to clear away excess material. This should be used if the material is too deep and/or hard to cut directly with your selected finishing tool. As documented above and below using this option with a flat shaped tool can also be very beneficial to the machining time and finish on cross section profile shapes with flat/horizontal regions.

When you use the option to Use Larger Area Clearance Tool, the software will calculate two toolpaths, the first will have [Clear] in its name to differentiate the two, [Clear] being the toolpath associated with the Use Larger Area Clearance Tooland the other, is the finish toolpath using the smaller tool. The [Clear] toolpath should be run first on the machine:

If this option is checked ✓ then the software will try to detect flat/horizontal areas in the cross section profile. If the specified Larger Area Clearance Tool can fit into these areas then they will be machined as part of the roughing operation. When using a flat tool this should give both a superior finish and also help to reduce the cutting time. Having this option checked ✓ will also allow you to choose the option Skip Flat Regions in the finish tool section which will stop the secondary toolpath from re-cutting these areas.

The machining allowance is a virtual thickness which is added to the moulding profile when the Use Large Area Clearance Tool is calculated. This ensures that the toolpath leaves some extra material on the part cut with a larger tool.

This option can be checked ✓ when working with rails that have sharp corners, allowing you to force the software to try and emulate these in the Moulding toolpath. Below you can see the effect of checking ✓ this option on a closed vector shape with the standard corners option on the left showing the toolpath rolling around the shape edge and the Sharp Corners option on the left where it has forced mitre style corners in the machined shape.

Moulding Toolpath - Create Sharp Corners Un-Checked

Moulding Toolpath - Create Sharp Corners Checked ✓

This option can be used to force the toolpath to cut past the edge of the part that is parallel to the drive curve vector. By default the center of the tool will go to the edge of the ends of the selected profile vector as its extruded along the drive rail. It may be desirable to extend this distance to either force the tool down the edge of the profile shape with vertical or steep edges or to ensure the toolpath has gone far enough past the edge to cleanly cutout the final shape with a profile toolpath. The value entered for the Boundary Offset will force the tool past the ends by the specified amount. As such if you want to ensure a vertical or very steep edge at your profile ends is machined you will need to specify a value which is at least the radius of your tool plus a small additional amount (say an additional 10% of the radius). For example if you are using a 0.25 inch (6mm) diameter ball-nose tool for the finish cut then you would specify a minimum of 0.15 inch or 3.6mm (= tool radius + 10%) to ensure the tool would be forced down the edges of your shape. If you wanted to ensure the roughing had also been able to machine these areas then the value should be based on your Larger Area Clearance Tool size instead.

This icon opens the V-Carving Toolpath form which is used to specify the type of carving required, details, cutting parameters and name for the toolpath.

V-Carving uses a constant angled cutter that's moved at flowing variable depth to create a 3D carved effect on the job. The software automatically calculates a path defined by the combination of the angle of the tool specified and the width and shape of the vectors being machined.

Watch this video to see this in action:

Checking ✓ this option limits the depth that the tool(s) will machine to, and is used for Flat Bottomed Carving and Engraving.

When No Flat Depth is specified the toolpath will be calculated to carve or engrave to full depth as shown below. Multiple z level passes will be automatically calculated where the tool needs to cut deeper than its Pass Depth specified in the Tool Database

No Flat Depth

Flat Depth

Flat Depth Using 2 Tools

Clicking the Select button opens the Tool Database from which the required V-Carving or Engraving 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. Note that Ball Nose tools can also be used to V-Carve designs.

Check ✓ this option if you wish to use End Mill, Ball Nose or Engraving cutters to machine the large open regions of a design. If no tool is selected here but Flat Depth is specified then the selected V-Carving tool will be used to clear the flat areas as well as for the V-Carving. All the tools in this section will leave an allowance for the V-Carving tool. Subject to this, the first tool in the list will remove as much material as it can, whereas subsequent tools will only machine areas the previous tools could not fit. The order of the tools in the list should match the order they will be run on the machine.

Clicking the Select button opens the Tool Database from which the required clearance tool can be selected and added to the list.

Clicking the Remove button will remove the selected tool from the list.

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.

Clicking the up and down arrow buttons will move the selected tool up and down the list respectively.

The strategy used to clear the material, either Offset or Raster, can be chosen for the first clearance toolpath. In the case of Raster, a Raster Angle can be entered.

The cutting direction, either Climb or Conventional, can be selected for each clearance tool.

Checking ✓ Ramp Plunge Moves applies ramping to the plunge moves of the clearance tool.

The above options are the same as those found on the Pocketing form.

Checking ✓ Corner Sharpen will raise the selected Engraving tool to fit the smaller tool tip into narrower regions. This option is available for a tool positioned second or later in the list.

If this option is checked ✓, the start point of the profile and offset toolpath segments will be as close as possible to the start point of the corresponding boundary vector. Otherwise this is left up to the program.

This option is only available if a 3D model has been defined. If this option is checked, ✓ after the toolpath has been calculated, it will be projected (or 'dropped') down in Z onto the surface of the 3D model. The depth of the original toolpath below the surface of the material will be used as the projected depth below the surface of the model.

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

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

Watch this video to see this in action:

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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

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

Watch this video to see this in action:

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

When this option is ticked,

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

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

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

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.

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

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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

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

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

Holding the 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.

Holding down altwith any of the above combinations will apply the kerning changes between every pair of letters on the line.

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.

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

Bend Text Upwards

Bend Text Downwards

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

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

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

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

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.

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.

Watch this video to see this in action:

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:

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

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

Clicking the color palette icon will pop up the Material Appearance dialog, allowing you to edit the appearance of the 3D shaded image for visualization purposes. The pull-down list offers a range of material types to shade the 3D model.

Additional materials can be added to the library using the list itself. You can add a category (folder) which groups your textures using <Create new category...>. You can also add extra textures under any category using <Add new texture...>.

Alternatively, you can copy an image file (JPG, BMP or TIF) of the material or image you wish to render the job with into the Textures folder within the 'Application Data Folder'. You can open the Application Data Folder from within the program using the File ► Open Application Data Folder menu command.

Shading textures can be obtained from sources such as the internet, clipart libraries or simply create your own from a digital or scanned photographs. For good quality results the image needs to be approximately 1000 pixels x 1000 pixels. The texture image is simply scaled proportionally in X and Y to fit the longest side of the job.

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.

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.

If this option is selected, each toolpath can have a different color assigned. If the 'No Fill' option is selected from the color picker form, the current toolpath will be shown in the material color.

Choose the color you want for the fill of that toolpath an

d 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:

Lithophane mode allows the preview to be shaded to give the effect of a semi-transparent material which is being lit from behind. The thinnest areas of material will appear brightest and then the brightness will be reduced to be lowest at the full material thickness.

Lithophane mode will work with whatever material or solid color is selected. The brightness of the material will vary between white at 0 material thickness and the selected color at full material thickness.

How a lithophane appears can vary depending on many factors including ambient lighting in the room, how strong the light behind the lithophane is and the properties of the material being used. The slider bar next to the lithophane option allows you to adjust the slider to account for these and to pick a value that looks right to you.

The below image shows the effect of changing the brightness slider. A white material has been chosen, as the slider increases from the left to the right the effect changes from being very high contrast to a much lighter appeance like you might see if no backlighting had been applied.

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;

This option animates all calculated toolpaths cutting into the material

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

Watch this video to see this in action:

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

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

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

Clearance less than Tool Diameter

Clearance greater than Tool Diameter

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

No Border Gap

Border Gap

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

Rotate Parts Enabled

Rotate Parts Disabled

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

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

Original

Parts Nested inside other parts

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

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

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

Double-sided part before selection

Double-sided part when selected

Select the vector you wish to use as the Filler Part, tick the "Filler" Tick box and click Apply to set this. The Filler Part Vector will be marked with a Green asterisk (*)

When the Nesting preview is applied, any area not filled by other nesting parts will be filled with as many Filler parts as can be made to fit in the remaining Sheet space.

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

Along X

Along Y

For more complicated nesting requirements it is possible to define how the nested parts are placed on to existing sheets and how new copies of existing sheets might be created to accomodate more parts. To edit the default setting click on the Customize button.

The Custom Sheet Selection form show the list of sheets we have to nest on to.

The slicing feature allows the user to divide the Composite Model into Z-Slices each of which will become a Component. This is for customers who need to cut a part which exceeds the Z depth of their machine gantry, the cutting length of their tools or the thickness of the material they are using. Once the slices have been cut on the CNC then they can be re-assembled to make the finished full depth part.

Watch this video to see this in action:

When this function is executed each slice will become a Component in the Component Tree and can then be moved into position and have toolpaths calculated on it. An example of this is shown in the images below, on the left it shows a scallop shell component that is 3 inches thick, the image below right shows this divided into two separate components, each a 1.5 inch slice of the original.

When the icon is clicked the Slice Model form will appear. This can be used to control the number and thickness of slices which will be created. At the top of the form it will display some reference information showing the thickness of the current Composite Model and also the currently defined Material Thickness (for machining).

The Model Slicing section can be used to set up the initial slices which can later be customized in the Slice Height section.

There are two ways to set up the initial slicing: by setting a standard slice thickness or by setting a fixed number of slices.

Checking ✓ this option will divide the model into a specific number of slices. The slice thickness will be determined by the Composite Model thickness divided by the Number of Slices defined. This may be a good option to use if the specific slice thickness is not important (for instance if it does not relate to material thickness).

Clicking Slice Model will apply the choices made in the form and create the Components which represent each slice of the Composite Model.

The Slice Heights section controls the specific details of each individual slice height. It also allows customization of the number of slices.

There are two parts to the slice height control:

• The height bar which gives a visual indication of the slice heights
• The slice list which lists the slice heights using their z value

The slice height section is for editing the values at which the model is sliced and not the slices themselves.

A specific slice height can be controlled by selecting it from the slice list, updating the value and clicking Apply

Additional slices can be added by either:

• Entering a specifc z height for the slice and selecting apply; or
• Double clicking on the height bar at a particular location

Double click to add slice

When the slicing tool is open then the 3D view gives a visualisation of the results of the slicing. If a slice height is selected then:

• Red areas show which are included in this slice
• Green areas indicate that the component is above the slice height and so these will be sliced flat.
• The slice will occur between the Red and the green areas.

Green areas are above the slice, red areas are the current slice.

You can also manuipulate the slices within the 3D View

• Double clicking on the model will change the value of the active slice height to be equal to the clicked height.
• Shift + Double Click will insert a new slice height at the clicked height.
• Shift + Mousewheel up/down will raise/lower the actice slice height by a small amount allowing you to tweak the thickness to remove thin slices.

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.

Watch this video to see this in action:

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.

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.

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.

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.

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

Loose

Tight

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 VCarve Pro parts (this is a rolling list that will be populated each time you run the software and may initially be empty).

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 VCarve Pro parts.

In the Startup Tasks section you will have the option to Create a new file, New file from template or Open an existing file.

Creating a new file allows you to 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).

New file from template will allow you to start a project using a pre-created template file from your computer. The CRVT3D or CRVT template files will have the necessary information for material size etc. already embedded in it. It may also contain vectors and toolpaths that have been created for this template file. Template file are created for settings you use regularly so you do not need to create them each time.

Open an Existing File, will allow you to open a pre-created file from your computer. This may be a file you previously created (*.crv3d or .crv). Alternatively, it might be a 2D vector layout from another CAD system (.dxf, *.eps, *.ai and *.pdf). A CRV3D or CRV file will have the necessary information for material size etc. already embedded in it. The 2D formats will import the data at the size and position it was created but will require you to go through the Job Setup form to verify/edit all the parameters for the part.

The Tutorial Video Browser will open your default web browser (typically Mircosoft Edge, 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.

We recommend you start with our dedicated Getting Started Videos that cover all typical beginner projects. Watch the first one here:

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

Watch this video to see this in action:

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.

If there are lots of vectors to trim then the left-click mouse button can be held down and then when the cursor is dragged and hovers over a vector then it will also trim the vectors. This can be much quicker than individually clicking spans.

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

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

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

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

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

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).

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

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

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

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

This section will present the process of importing the Full-3D STL model into rotary project, using a table leg as an example.

There are two basic use cases when importing an external model into the rotary job. The first case involves bringing a model designed for this particular job in another software. Thus the dimensions of the imported piece may already be correct and it can be desired to use them for the size of project. The second use case is when importing a stock model that would have to be scaled to fit on particular machine.

Aspire uses following workflow that covers both of those cases:

1. Setting-up rotary project
2. Choosing file for import
3. Orientating the model in material block
4. Scaling the model
5. Finishing the import

Create a new job using the Job Setup form. It is important to set the job type as rotary to ensure a proper import tool is used in the next step.

If the dimensions of the project are already known, they could be specified directly.

If it is desired to fit the model to a given machine or stock available, set both the diameter and length to maximum. During import the model will be scaled to those limits.

If it is desired to use the imported model size, any size can be specified at this time. During the model import the project can be automatically resized to match the model dimensions.

In this example it was desired to fit the model into a specific stock size with a Diameter of 4 inches and a Length of 12 inches. XY origin was set to centre.

To start the importing process, use Import a Component or 3D Model tool from the Modelling tab

Make sure that the Imported model type is set to Full 3D model .

The first step is to position the imported model within the material. This step is necessary as this information is not present in the imported file. When the model was opened, the import tool chose the initial orientation, as can be seen below.

To help with orientating the model, the software displays a blue bounding cylinder. This cylinder has the rotation axis aligned with that defined for the material block and thus can be used as a reference. Its size is just big enough to contain the imported model at the current orientation. When the model orientation is changed, this blue cylinder will shrink or grow so it always contains the model. At this stage its exact dimensions are not important, as we are only interested in positioning the model correctly.

The software also highlights the rotation axis in red. This is particularly important when importing bended models. It is currently not possible to represent areas of model that are entirely below or above the rotation axis. This is the case in the example shown here. If the model was imported as is, the distortion would be created as can be seen below. Therefore it is important to position the model in a way such that the rotation axis is contained within the model.

The last guiding element displayed by the software is the red half arrow on the side of the cylinder. This arrow is indicating the position that corresponds to the center of the wrapped dimension in the 2D view. In this example the model is orientated in such a way, that front of the leg would be placed on side of the 2D view, rather than centre. Thus it is better to rotate model so this arrow points to the front of the imported model.

The import tool provides a few ways of adjusting the model orientation. The most basic one is the Initial Orientation. This can be used to roughly align the model with the rotation axis. This can also be combined with the Rotation about Z Axis.In this example the tool chose Left with no rotation. In order to align the front of the leg with the red arrow, one could use the Front and -90 as the Rotation about Z Axis.

Once the initial orientation is decided, further adjustments can be made using the Interactive Rotation. The default option - XYZ View - disables the interactive rotation. That means that the 3D view can be twiddled with a mouse. Selecting other options enables the rotation around the specified axis.

In this example, instead of changing the initial orientation to align the front of the leg with the red arrow, one could select X Model option and rotate the piece manually. When selecting single axis rotation, the 3D view will be adjusted to show that axis pointing towards the screen. If any mistake is made, it is possible to undo rotation using Ctrl+ Z

Notice that whenever the part is rotated, it is always centered in the cylinder. In this example it is not desired, since we need the rotation axis to be contained within the model. In order to move the model in relation to the rotation axis, one can use the Rotation Axis Movement

Similarly to the previously described tool, when Rotation Axis Movement is set to Off, the 3D view can be panned

Correctly positioning the model for importing may require a combination of the Rotation Axis Movement and the Interactive Rotation to achieve desired results with models that bend. It is important to make sure that rotation axis is hidden in order to avoid distortion. However it is also desirable to have the rotation axis being in the center of each segment of the piece to ensure tool has angle close to the optimal during machining. Usually it is also useful to rotate the model in view around the axis after the adjustment, as this allows us to inspect the model from each side without the need to disable the Interactive Rotation before changing the viewing angle.

It is important to understand that Aspire does not support 4-axis machining. That means that while the machined piece can be rotated and tool moves along the rotation axis and in the Z direction, it is not possible to move the tool in the wrapped dimension and thus the tool is always above the rotation axis and cannot be moved to the side.

This limitation is shown below. The first picture presents correct machining of the point. If the tool moves to another location though, the angle will be incorrect and even worse, the tool side will be touching the stock.

3-axis rotary machining, tool correctly positioned

3-axis rotary machining, tool side is touching the stock

Once model has been positioned as desired, its size can be taken into account.

By default the tool will assume that imported model is using the same units as the project. If that is not the case, model units can be switched. In this example project was set-up in inches, while imported model was designed in mm. After switching model becomes considerably smaller and a red cylinder, representing current material block is shown, as can be seen below.

At this point it is possible to specify the model size, in terms of diameter and length. This can be done manually by typing desired dimensions, or by fitting to material. If Lock ratio option is selected, the ratio between diameter and length is kept. One can also tick Resize material block option. If it is selected, the material block will be scaled to match current size of the model, after OK is clicked.

If it is desired to use model size as material block size, one can just make sure units are correct, then tick Resize material block option and press OK.

If it is desired for the model to fit material, one could click Scale model to fit material and tick Resize material block.

In this example model was fitted to material. Since in this case length of the piece is limiting factor and lock ratio is maintained, this results in model having considerably smaller diameter than material block. Hence Resize material block option was ticked.

After pressing OK the model will be imported as a component. It is possible to modify it as any other component or add pieces of decorative clipart onto its surface if desired.

It is important to keep in mind the distortion caused by the wrapping process. That means that wrapped toolpaths will match flat toolpaths only at the surface of the blank. The closer to the rotation axis (i.e. deeper) the toolpath is, the more it will be 'compressed'. This fact have a profound implication for 3D toolpaths. Consider the example shown below.

As can be seen if there is substantial difference in diameter in different parts of model, generating one 3D toolpath for whole model will result in wrapped toolpath being overly compressed. Thus it is usually better to create boundaries of regions with significantly different diameter and generate separate toolpaths using correct settings for each diameter.

This section will present a process of importing Flat STL model into rotary project. Flat models are similar to decorative clipart pieces provided with Aspire and are supposed to be placed on the surface of modelled shape.

To start the importing process, use Import a Component or 3D Model tool from the Modelling tab

Make sure that Imported model type is set to Flat model

Again the first step is to select proper orientation of model. The tool will chose initial orientation and display model in the red material box. This box corresponds to the 'unwrapped' material block and its thickness is equal to half of the specified diameter of the blank.

If model is not oriented correctly, that is, does not lie flat on the bottom of the material box, as can be seen above, orientation have to be adjusted. To do that one can change Initial Orientation option and/or Rotation about Z Axis.

If imported model is not aligned with any of the axes, it may be necessary to use Interactive Rotation.The default option - XYZ View - disables interactive rotation. That means that 3D view can be twiddled with a mouse. Selecting other options enables rotation around specified axis.

Each rotation can be undone by pressing Ctrl+ Z.

Once model is properly orientated, units conversion can be performed. By default the tool will assume that imported model is using the same units as the project. If that is not the case, model units can be switched.

There is also model scaling option included. When Lock ratio option is selected, the ratio between X, Y and Z lengths are kept. Note that once model is imported, it will be added to project as a component. Hence correct placement, rotation and sizing can be performed later, after model is imported.

If the project does not contain any models yet, following message will be displayed:

Typically you could simply click Yes.The more detailed explanation about modelling plane adjustment has been provided in Modelling 3D rotary projects

In the unfortunate event of the software crashing,

1. We try to save unsaved changes, so that your data isn't lost.
2. Provide an easy way for you to report the crash so that we can work on a fix.

You will need to be connected to the internet for this to work. If not, you can still send the generated zipped report to support@vectric.com. The report can be found in the Application Program Data (Accessible through the menu File ⇛ Open application data folder.... If you try to send the report and it fails, you will get a message of where that path is and possible methods to get that report to us.

The crash reporting is powered by BugSplat (a third-party) company which provides us with the tools that help us analyse them.

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

Watch this video to see this in action:

This slider adjusts the contrast.

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

A lower contrast will reduce that difference and make the image more neutral and average.

Rectangular Border

Oval Border

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

Rectangular Border

Oval Border

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

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

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

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

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

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

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

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

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.

Watch this video to see this in action:

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.

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

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

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

Example

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

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

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

Examples

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

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.

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

This window allows you to view the contents of the selected post-processor file.

This can be viewed from the Machine Configuration Management dialog and costomized through the Post-Processor Management dialog.

To view, open the Machine Configuration Management dialog, click on the post processor that you wish to view with the Right hand mouse button and select "View" from the right hand click menu.

Please note: The view option is not available for custom post processors that you have placed in your My_PostP folder.

You can cut and paste content in text form to the clipboard of your computer.

Within the Post-Processor Management dialog form you can mark a post processor as being a custom one. To do this click on the Edit icon

This will move the selected post processor to your My_PostP folder. You can make edits to this post processor with any text editior.

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

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

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

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

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

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

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

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

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

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

The manual method allows entry of license details without requiring an Internet connection.

There are 2 methods for entering a licences,

1. Loading from a File
2. Typing or Copying the values into the text fields

You can choose to download a vlicence file from your V&Co account.

There are 2 ways to use this file

1. Double-click the file to open it with the software
2. Go through the License Dialog wizard and click to Load the vlicence file.

License Data

You can get the License Data from your V&Co account and enter it using the Enter License Data option.

Registered User Name & License Code

If you are not registered but you have received a Register User Name and License Code with your recently purchased machine, then you can enter those using the Enter User Name & License Code option.

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

Pressing Next > will set the license and display the summary screen.

Adding Module

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

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

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

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

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

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

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

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).

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

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

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

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

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.

Watch this video to see this in action:

CNC machines that require the tooling to be changed manually will typically need a separate toolpath for each cutter used. The procedure for saving this type of toolpath is to:

• Select the toolpath to save from the Toolpath List
• Click on the Save option and the Save Toolpaths form is displayed.
• Select the desired Machine from the pull-down list.
• Select one of the Postprocessors associated with that machine from the pull-down list.
• Click the Save Toolpath(s) button.
• Enter a suitable Name and click the Save button.

When Machine is selected from drop-down list, the Postprocessor list is updated to only show those relevant for the selected machine. Before this can happen Postprocessors have to be associated with given machine.

The Postprocessors can be associated with Machine using Machine Configuration Dialog that can be accessed by clicking on

You can also select <Add Post-Processors> option from the Postprocessor drop-down list to quickly associate Postprocessors with currently selected machine.

For more details please refer to Online Machine Configuration and Manual Machine Configuration.

Saves all of the visible toolpath to individual files. You will be prompted to provide a filename. This filename will be used as a prefix for each of the files.

If the option Group where possible is chosen then consecutive toolpaths which use the same tool will save out to the same file. In this case then the chosen name will be applied, as well as numbers which indicate which toolpaths have been saved. For example, if you decide to name your files Toolpaths and the first 3 toolpaths can be all output in single file, then that file will begin: Toolpaths_1-3 to indicate that it is toolpaths 1- 3 which are being saved out.

CNC Machines that have Automatic Tool Changing (ATC) capabilities can work with a single file that contains multiple toolpaths, each having a different tool number.

The postprocessor must be configured to support ATC commands for your CNC machine. Contact your software or machine supplier for more details.

• The procedure for saving these toolpaths is,
• Use the Up and Down arrows to order the toolpath list in the cutting sequence required.
• Tick each toolpath to ensure it is drawn / visible in the 3D window as shown:
• Click on the Save option and the Save Toolpaths form is displayed. Select the option Output all visible toolpaths to one file

The names of the toolpaths that will be written into the file are displayed along with the tool number in square brackets [1]. If a calculated toolpath is not required, simply tick to undraw it.

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

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.

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

Watch this video to see this in action:

Switch between standard Text tool and Text in a Box Tool modes.

To enter text:

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

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

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

The Standard Text tools are replaced with specialist Text In a Box tools.

Watch this video to see this in action:

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.

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

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

To edit text properties or content of previously created text:

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

The Text tool has a spell checking feature to assist with spelling errors.

• The software checks the spelling for the user and underlines the misspelled words with red.
• When an underlined word is clicked. It suggest corrections for the user.
• There is an add word feature if you want to add a new word.
• There is a remove word feature if you want to remove a word you added by mistake ( it has to be a word added by the user).
• The language of the spell checker is the same as the language of the software.
• All the Software supported languages are supported by the spell checker except for Japanese

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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.

Watch this video to see this in action:

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.

When a toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description) is used to determine the number of passes needed to profile down to the specified Cut Depth. However, by default the software will also modify the precise step down by up to 15% in either direction, if by doing so it is able to total number of passes required to reach the desired cut depth. It is nearly always desirable to benefit from the significantly reduced machining time of cutting using less passes if possible. Nevertheless, there are some occasions where the exact step down for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section page indicates how many passes will be created with the current settings.The Edit Passes... button will open a new dialog that enables the specific number and height of passes to be set directly.

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.

The first method simply sets the passes based on the Depth of Step property of the selected tool. By default, this is the method used by Aspire when initially creating profile passes. However, if the Maintain Exact Step Depth option is checked, the software will not vary the step size to try to optimize the number of passes (see above).

The second method creates evenly spaced passes based on the value specified in the Number of passes edit box.

To apply either method, click the Set Associated Passes button to create the resulting set of pass depths in the pass list and diagram.

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

Outside

Inside

On

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.

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.

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.

When this option is selected the tab will be triangular in section. This is shape is created as the cutter ramps up to the specified Tab Thickness then down the other side. The 3D Tabs will often allow the machine to run quicker and smoother because it does not have to stop to move in Z at the start and end of each tab.

3D Tab

If this option is unchecked, the 2D tabs will be used. The cutter stops at the start point for each tab, lifts vertically by the specified Thickness runs across the ramp, stops and plunges down the other side.

Tab thickness is measured from the bottom of the CUT DEPTH, not the Material bottom.

How the lenght and thickness change the tab size

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.

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.

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.

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.

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.

This option creates an arc lead onto the toolpath using the Radius and Lead length distance specified.

The Radius and Angle will automatically inform the Length when entered, and the angle range is 0.1 to 90 degree.

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.

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.

This option is only available if a 3D model has been defined. If this option is checked, ✓ after the toolpath has been calculated, it will be projected (or 'dropped') down in Z onto the surface of the 3D model. The depth of the original toolpath below the surface of the material will be used as the projected depth below the surface of the model.

The Chamfer Toolpath uses the selected vectors and tool to create an angled feature

The Chamfer Toolpath has two distinct ways of operating depending on the tool used:

• If the selected tool is an angled tool, then the angle of the tool determines the angle of the chamfer
• If the selected tool is a round nosed tool, then the angle of the chamfer must be specified manually, and will be approximated by a series of fine cuts.

Watch this video to see this in action:

The angle determines the slope of the chamfer. It is measured from vertical.

When a V-Bit tool is selected for the toolpath then the angle is fixed to half of the angle of the tool.

For a round nosed tool then the angle may be specified.

To achieve the desired height of the chamfer, as specified by the cut depth field, cutting deeper might be required. This will be true in the case of a round-nosed tool.

The Max Cut Depth field is read only and shows the full length of the cut so you can accurately see how deep the tool cuts.

When using a V-Bit tool for chamfering it can be desirable to use the edge of tool, and keep the point of the tool off the part. Small movements in the machine and the material can mean that the point of the leaves an unsightly witness mark. The overcut control allows you to specify a value that will be used to offset the centre of the tool, and use the side of the tool for machining.

The overcut distance offsets the tip of the tool. It also makes the cut deeper

The Chamfer Type option controls whether or not a chamfer occurs inside or outside a vector and the direction of the chamfer slope :

• An inner chamfer will be inside the selected vector.
• An outside chamfer will be outside the selected vector.

The direction of the slope tells us whether our chamfer is upward or downward relative to the selected vector or whether it is downward relative to the selected vector.

Chamfer Outside & Down. With pocket clearance outside

Chamfer Outside and Up. Clearance pocket inside the vector

Both options can be used together to generate different chamfer styles.

When using the Chamfer toolpath the 2D View will provide immeditate feedback on what the resulting chamfer will look like. Small lines will extend outwards from the selected vector to show where the slope of the chamfer will lie. The arrows on these line indicate the direction of slope. The arrows always point down in the direction of the downwards slope.

2D Preview Showing Chamfer Outside the vectors. The directions point in the direction of the downwards slop.

Result of Chamfer Toolpath when previewed

When you load a previously saved toolpath template (using Toolpaths ► Templates ► Load Template...) you will have an empty toolpath which can be edited by double clicking on its name in the toolpath list or selecting the Edit Toolpath icon in the Toolpaths tab. Once the toolpath form is open, the vectors to be machined can be selected and the toolpath calculated using all the saved settings.

If you load a toolpath template which has toolpaths associated with layers which don't exist in the current file, the Missing Layers for Template dialog will be displayed. It lists all the missing layers and offers you the choice of having them created automatically, deleting toolpaths associated with missing layers or just loading the toolpaths as is.

Choosing to allow the dialog to automatically create the missing layers allows a toolpath template to be used to create 'standard' layers for machining operations and load the toolpaths ready to be calculated. All you then need to do is move vectors to the appropriate layers and recalculate all the toolpaths.

Choosing the Delete all toolpaths associated with missing layers option allows you to create a single template with many toolpaths and have the ones which aren't appropriate to the current job automatically deleted.

The nature of different styles of toolpaths means that they may be simple 2D cuts or require simultaneous 3-axis moves, the more complex the toolpath then the more chance the CNC machine may not actually achieve the programmed feed rates. This can be compensated for by multiplying the times by the Scale Factor.

The scale factor in the program lets you approximate this slowdown for your machine, but it will vary depending on the type of work you are doing. Many people will use one scale factor for simple 2d work and another for 3d or VCarving. The best way to calculate it is just to take a note of estimated and actual machining times of a period of time.

For machines where the controller provides an estimated machining time, these should be more accurate as the controller can determine where the machine is accelerating / decelerating and take account of this.

Notes for the summary of the toolpath can be written here.

Click Apply once written to store them.

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

When there are multiple sheets in the job then the outline of the sheets is shown in the 2D view.

Here you can see Sheet 1 Is the Active Sheet.

When vectors lie outside of the bounds of a sheet, then the bounds in the 2D view are updated to indicate this.

A sheet can be activated by using the Sheet Management Tab, using the Sheets Dropdown menu, or by double clicking on the sheet in the 2D view.

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

Watch this video to see this in action:

• 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.

• 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.

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:

Different form is displayed depending on the job type:

• Single- or double- sided job,
• Rotary job.

Watch this video to see this in action:

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 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.

Instead of cutting a series of individual pieces of material and assembling them later, it can also be convenient to cut a single strip of material using a series of set-ups - moving the material through the machinable area between cuts. Aspirespecifically supports this technique using the Feed-through in X/Y options. In these cases you will only need to define either the Tile Width or Height (which corresponds to your intended feed-through distance), as the other dimension is assumed to correspond to the shorter side length of your material and will match the equivalent current job dimension. Similarly, the overlap distance is only applied in the direction of the draw-through. Because you will typically be cutting the same piece of material with each toolpath tile, the overlap distance for Feed-through is not as critical as for Individual tiles and is typically used to allow for a margin of error in your set-up accuracy.

Once you have set your tiling option, click the Update Tiles button to see your settings reflected in the Tile Previews in either the 2D or 3D Views.

The 2D View indicates how the model area is split into tiles. The yellow lines indicate the tile sizes, but the light red areas also indicate the overlap region for each tile.

Double-clicking on a tile will make that tile the active tile.

In the 3D view the toolpaths will be showed tiled, with only the moves that are within the active tile shown.

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.

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.

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 VCarve Pro 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 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 VCarve Pro, such as describing a shape for a toolpath to follow or creating designs. VCarve Pro 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. VCarve Pro 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.

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 Work with, VCarve Pro 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.

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

Watch this video to see this in action:

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:

Transform Handles

When in this mode the mouse is used to click on one of the handles which has appeared on the selected Vector/s. Each Transform handle is used for a specific editing operation as detailed here in the 2D View:

• Middle - Move the vectors (Hold +Alt Move the selected objects in one axis)
• Middle - Click a second time to switch to Rotational center. Click and drag the Rotational Anchor to reposition the Rotational Center of the current selection.
• Corner (White) - Scale the vectors proportionally (Hold +Alt Scaling non-proportionally, +Shift Scale around the centre)
• Edges (White) - Scale the vector in one axis (Hold +Shift Scaling proportionally)
• Corner (Black) - Rotate the vectors (Hold +Alt Rotate in 15° increments) about the Rotation Center.

To deselect objects,

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

In the 3D View, the Transform Handles are:

• Middle - Move the vectors (Hold +Alt Move the selected objects in one axis)
• Middle - Click a second time to switch to Rotational center. Click and drag the Rotational Anchor to reposition the Rotational Center of the current selection.
• Corner (White) - Scale the vectors proportionally (Hold +Alt Scaling non-proportionally, +Shift Scale around the centre)
• Edges (Black) - Scale the vector in one axis (Hold +Shift Scaling proportionally)
• Rotation Arrow (Top Black) - Rotate the vectors (Hold +Alt Rotate in 15° increments)

When you select a Transform Handle, it will activate the appropriate Edit Box for that Handle.

If you need an exact value for a Transformation, click into this box and type in the desired value, followed by Enter to accept the new value.

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

This tool uses the differences in contrast between areas of a Bitmap image or a 3D model to create a toolpath and create a Sketching style carving design of the outline.

Original 3D model

Sketch Carve Result

Watch this video to see this in action:

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.

Allows a vector to be used as a boundary to limit the extent of the toolpath creation.

Hold SHIFT and selected the desired Vector to use as the boundary after selecting the Bitmap or 3D model you are Sketch Carving.

The Line Thickness slider will allow you to adjust the weighting of your sketch lines created from your 3D model or Bitmap image.

This can slide between 0 and 100.

The higher the value the thicker and heavier the sketch carve lines will be but the less detail will be picked out.

100 Line Thickness

0 Line Thickness

You can see here the green hightlighted area shows the area which will be cut in this toolpath, with the lower Line Thickness picking out more lighter details, but overall cutting a much shallower area, while the Thicker Line Thickness will apply more heavily to the largest areas while not cutting the finer details.

By reviewing the Sketch Carves Green Highlights you can get a good idea how the toolpath will cut before calculating it.

This option is only available if a 3D model has been defined. If this option is checked, ✓ after the toolpath has been calculated, it will be projected (or 'dropped') down in Z onto the surface of the 3D model. The depth of the original toolpath below the surface of the material will be used as the projected depth below the surface of the model.

In addition to the pre-set Variables list, the user also has the option to define their own custom Variables which may use other attributes of the tool that are not possible to include within our default tool naming convention. This could then be used to better assist the user in distinguishing one tool from another at a glance. For example, you could choose to include the tool manufacturer, purpose and material as a variable which can be applied to individual or full groups of tools.

The Custom Attributes variables form is accessible from within the tool database.

1. Open the tool database through clicking the tool database button within toolpaths panel or though; Toolpaths (In menu bar) > Tool Database

2. Select the specific tool you would like to create custom Variables for and then Click The ‘Variables’ button to the Right of the notes field in the main tool geometry section of the form, to open the ‘Custom Attributes Variables’ form.

3. At the very top of the form under ‘New Variable’ you will see two edit boxes;

• Name – This is the title of the Variable, and specifies the expression you would need to enter within the tool name field to achieve the required Value.
• Value – This is the resulting text which replaces the corresponding user defined expression when entered into the tool name field.

This means that if you require X Value within the tool name then you would need to enter Name Y within curly Brackets {Y}. Y is defined by the Name field of the Custom attributes Variables form.

4. Click the ‘Create’ button to the right of the edit boxes to apply changes and to create the custom variable, then Okay to close out of the form.

1. Click the ‘Edit’ button next to the tool name above the notes field.
2. Place cursor where you would like to place value within string
3. Right click > Custom Attributes variables > Search and select correct name in list.

• Click ‘Ok’ at the bottom of the form to apply changes.

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

It also allows image files to be selected and imported into the current open job. File types - BMP, JPG, TIF, GIF, PNG

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

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

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

This section will show how to create a simple column, using the profile and fluting toolpaths.

Start by creating a new rotary job. Please note that settings shown here are only an example and should be adapted to match your machine setup and available material.

In this example the blank will rotate around X axis. We will refer to it as the rotation axis. The axis that will be wrapped is the Y axis. We will refer to it as the wrapped axis. That means that the top and bottom boundaries of the 2D workspace will actually coincide. We will refer to them as the wrapped boundaries.

First, create the cove vectors using Draw Line/Polyline tool. Those will run along the wrapped axis at both ends of the design. Snapping may be useful to ensure that the created line starts and ends at the wrapped boundaries.

In this example the coves were placed 1 inch from the job boundaries, leaving 10 inches in the middle for the flutes. The flutes will run along rotation axis. Assuming 0.5 inch gap between the cove and the beginning of the flute, the flutes will have the length of 9 inches. This example will use 8 flutes.

To start, create a line parallel to rotation axis that is 9 inches long. Now select the created flute vector and then select one of the cove vectors while holding down Shift. Then use Copy Along Vectors tool to create 9 copies. The original flute vector may now be removed as it is no longer necessary. Note that first and last copy are both created on wrapped boundaries. That means they will coincide, so one of them can be removed. As the last step select all flute vectors and press F9 to place them in the center of design.

The process of creating 2D rotary toolpaths is very similar to creating toolpaths for Single - and Double - models. This example will use the profile toolpath on the cove vectors. To create the toolpath, select the cove vectors and click on the Profile Toolpath from

To create the toolpath for the flutes, select the flute vectors and click on the Fluting Toolpath. This Example used a 1 inch 90deg V-Bit set to Flute Depth 0.2 and using the Ramp at Start and End and Ramp Type Smooth options. Ramp length was set to 0.25 inches. Both toolpaths can be seen below.

It is time to simulate toolpaths using Preview Toolpaths. If the option to animate the preview is selected, the simulation will be visualized in flat mode. Once the simulation is complete, the wrapped rotary view will be turned back on automatically.

Although the design can be considered to be finished, in practice it is useful to be able to cut-out the remaining stock. This can be realized by making the design slightly longer and adding profile cuts. In this example the blank length was extended by 2 inches using the Job Setup . Existing vectors can be recentered using F9After that the existing toolpaths have to be recalculated.

The cut-out vectors can be created in the same way as cove vectors. Two extra profiling toolpaths can be created using the suitable End Mill. In this example we used a tab with a 0.5 inch diameter. In order to achieve that, the user can type the following in the Cut Depth box: z-0.25 and then press = and the software will substitute the result of the calculation. Variable 'z' used in the formula will be substituted by the radius of the blank automatically by software. It is also important to specify Machine Vectors Outside/Right or Machine Vectors Inside/Left as appropriate. The cut-out toolpaths and the resulting simulation can been shown below.

Cut-out toolpaths in 2D view

Finished part after adding cut-out toolpaths

The final step is to save the toolpaths in a format acceptable by your machine. Use the Save Toolpaths and select the wrapped post-processor matching your machine.

This section will explain how to create and simulate spiral toolpaths.

One way of thinking about spiral toolpaths is to imagine a long, narrow strip of fabric. Such a strip can be wrapped around a roll at a certain angle. In order to create a toolpath that wraps around the blank multiple times, one can create a long vector at a certain angle. Such a vector is an equivalent to the strip of fabric when it is unwrapped from the roll.

Although such a toolpath will exceed the 2D workspace of the rotary job, thanks to the wrapping process during both simulation and machining the toolpath will actually stay within material boundaries.

The most crucial part of designing spiral vectors is to determine the right angle and length of the line that would result in a given number of wraps. Suppose one would like to modify a simple column design to use spiral flutes, rather than parallel to rotation axis. The following example will use flutes wrapping 3 times each, but the method can be adapted to any other number.

All but one of the existing flute vectors can be removed. Select the Draw Line/Polyline and start a new line by clicking at one end of the existing flute. This line needs to be made along the wrapped axis with the length being 3 times the circumference of the job. In this example that means typing 90 into the Angle box and typing y * 3 into the Length box and pressing =. If the wrapped axis is not the Y axis, but rather the X axis, then the above formula should be x * 3.

Now one can simply draw a line connecting to the other end of the original flute vector and the newly created one. Using Copy Along Vectors tool this single flute may be copied in the way described earlier. In this example 4 spiral flutes were created, as can be seen below.

Vectors used to create spiral flutes

Spiral toolpaths in flat view

Once the flute vectors are ready, the toolpath can be created again using the Fluting Toolpath. An important thing to note, is the difference between the appearance of spiral toolpaths in the wrapped and flat view. By clicking on Auto Wrapping one can switch from wrapped rotary view to flat view and back again.

As can be seen above, in the flat view the toolpaths will follow the vectors and extend beyond the job boundaries. On the other hand the wrapped view, presented below, will display the toolpaths spiralling around the blank.

This was just a brief overview of general 2D workflow for rotary machining. Remember to also take a look at video tutorials dedicated to rotary machining, which are accessible from the Tutorial Video Browser link when the application first starts.

We are providing a selection of prepackaged machine configurations for the most popular machine manufacturers and the list is continually growing.

This will take you to the Search Machine Online dialog. If you find and download your machine, it will be imported into your tool database with some initial feeds and speeds for a set of tools. It will also be associated with the post-processors compatible with it.

This can all be done or edited later on through the Machine Configuration dialog.

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 MenuView Menu ► Guide Lines ► Delete All Guides from the Main Menu

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

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

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

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

Snap to Nodes, mid-points, centers

Snap to Guides, matching horizontal and vertical points, plus angle and distance

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	Description
	Object Bounds	The theoretical bounding box surrounding the active vector + horizontal and vertical lines passing through the centre
	Horizontal and Vertical Lines	Horizontal and vertical lines passing through a node or a span midpoint.
	Tangents	Tangents originating from a node or a span midpoint.
	Perpendicular to Tangents	Lines which are perpendicular to tangents from nodes or span midpoints.
	Connecting Lines	Lines connecting two nodes. Includes mid-point.
	Span Geometry	Snap to the geometry of the vector.
	Angular Constraints	Snapping to specific angles, as defined in the snap options F4.
	Job	Horizontal and vertical lines through the center of the job.

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

Bounding Box

Object Center

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

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

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

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.

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

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.

The start and end points can be aligned horizontally or vertically while the vector is being rotated.

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.

The Vectric Workflow

The Example Project will step you through all the stages of creating, toolpathing and cutting a simple line drawing. Most CNC projects share many common concepts and steps so before we complete our practical project, let's run through them.

The structure of a Vectric Job

All the information needed to describe a single CNC project is contained in a Vectric Job document (when saved they have the file suffixes *.crv or *.crv3d). A new job always begins by defining the area of a sheet of physical material that you intend to cut with your CNC machine.

Most jobs typically only involve one sheet of material, but more complicated projects may comprise multiple materials. Don't worry, your job's primary material sheet can be updated or new sheets of material added to your job later, as your design develops.

The drawings & images used to work on a material sheet can be created on layers to help manage more complicated designs. Similarly 3D model components can also be organised onto levels. By default there is always at least one layer and one level for each sheet in a new job. You can add more layers and levels to help organise more complicated projects.

Once your material sheet has been created in the Job Setup form, the software will show you a 2D & 3D view of your design space (which matches the dimensions of your current material sheet), each in their own window.

Above the view windows is the main toolbar which allows you to navigate through the structure of your CNC job and see what is currently being displayed in view windows below. It shows you the material sheet, design layer and 3D model level that you are currently working on (referred to as 'active').

What you see in the 2D & 3D design views below will reflect these current settings and any new shapes, components or toolpaths will be created in the active locations indicated. You can also change the active sheet, active layer or active level at any time directly from these controls.

More advanced projects can also represent both sides of a sheet of material. For a two-sided project an additional control above the views shows which side of the sheet is currently active. You can view the drawings, models and toolpaths associated with the top and bottom surface of each material sheet and swap the active side of the sheet in a consistent way to the other controls.

Initially your job will be empty and so your views will be blank, but in due course, Vectric's view windows will show all the layered drawings & images, 3D model components & toolpaths for the currently active material sheet.

The currently active locations are the same for both the 2D & 3D views i.e. creating a vector shape will place it on the same active sheet and active layer regardless of whether the 2D or 3D view is used.

You can, however, toggle the visibility of object types in each view independently using the visible items toolbar at the top of each view. This is helpful for focusing on different areas of your job at each stage of creating your CNC project.

Many of the software's tools can be used directly in either the 2D or 3D view.

In V12 some tools have not yet been extended to allow full interaction in the 3D - this is an ongoing transition. If in doubt, try click

Import, Draw or Trace artwork

Computer images are most often represented as a grid of coloured squares - these images are referred to as bitmaps and their constituent coloured squares are called pixels. Except for a few very specific cases, this representation is not *directly* useful for toolpath creation. Computer drawings (from CAD or illustration applications) are very different and are instead built from mathematically defined lines & curves.

This type of representation is referred to as vector or contour artwork. Vectric software can use both bitmap and vector artwork, but most types of toolpath can only be created from vector drawings. Suitable bitmaps with bold regions of similar colour (for example logos, cartoons, icons or signs) can, however, be used to create vectors from which many types of toolpath can then be generated - this process is called bitmap tracing.

Some external artwork file types contain only bitmaps (e.g. BMP, PNG, JPG), some contain only vectors but many can contain both (e.g. PDF, SVG, DWG/DXF).

Use the design artwork to create toolpaths

We use the vector artwork to define the shapes we want to cut. It is important to emphasise that the toolpath (the actual cutting moves your machine must make to leave your intended shape) is rarely, if ever, a direct conversion of the original artwork. The toolpath must be created taking into account a complex interaction of the material, your CNC machine's capabilities and the shape of your cutting tool.

"Sculpture, per se, is the simplest thing in the world. All you have to do is to take a big chunk of marble and a hammer and chisel, make up your mind what you are about to create and chip off all the marble you don’t want." - Paris Gaulois, 1879.

Toolpaths are therefore generated from source vector artwork but once created they are almost entirely indepenendent of the artwork that created them. Moving, editing or even deleting the source artwork used to generate a toolpath will not affect the toolpath - it must be actively re-calculated to reflect any changes.

This is a carefully considered Vectric design principle - although you may be prompted that a significant alteration to your job has occurred - your toolpaths will never change automatically 'behind your back'!

That said, toolpaths do retain a handy reference to the artwork that created them. If you choose to edit a toolpath it will try to locate it's orginal source artwork and re-select it. At this point you can simply recalculate it to reflect any changes you have made to that source artwork, but you can also choose to select additional or entirely different artwork.

Preview

As we've discussed, the actual motion of your CNC machine (the toolpath) required to cut al shape can be complex and difficult to interpret.

Luckily your software provides an extremely accurate preview of any toolpaths that you create by simulating them in a block of virtual material. In the Example Project we will use the Toolpath Preview to verify that the toolpaths are producing the shapes we want (and we can easily corrected them if not)!

This simulated preview is a hugely beneficial step that ensures you minimise costly mistakes in the real world (we all make them from time to time) but it also allows you to check the surface finish you can expect from different strategies under different conditions.

The Toolpath Preview uses exactly the same data that will be sent to your CNC machine. You can be confident that any cutting and surface finish issues that occur at the machine but which are not visible in the Toolpath Preview are almost always caused by a physical problem with the machine setup or tooling, which makes finding and fixing them a lot quicker!

Exporting the toolpath

Now we will be ready to export the toolpath, in the right format, ready to be loaded into our CNC machine's controller. Saving the toolpath will make use of a Post-Processor that is specific to your CNC machine. It will translate the movements contained in the toolpath into a toolpath file that is in the specific format required by your CNC machine's controller to load and run.

• This allows you to add notes to your file/model.
• If the notes start with . the notes section will auto open when you open the file with which they are associated.

There is also a spell checker features attached to that.

• The software checks the spelling for the user and underlines the misspelled words with red.
• When an underlined word is clicked. It suggest corrections for the user.
• There is an add word feature if you want to add a new word.
• There is a remove word feature if you want to remove a word you added by mistake ( it has to be a word added by the user).
• The language of the spell checker is the same as the language of the software.
• All the Software supported languages are supported by the spell checker except for Japanese

HTML Links.

To enter a link into the Note, go to the appropriate page in your Web Browser and select the URL of the page from the Address Bar.

CRTL+C to copy it and then in the Note Field, right click and use the "Paste" option to enter it into the Notes.

To use the HTML Link in the Note Window, hold the CRTL Key and click the link. This will open your computers default Web Browser and load the web page.

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.

Watch this video to see this in action:

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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

See Grouping and UnGrouping.

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.

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

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

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

Watch this video to see this in action:

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

The model that you see in the 3D View is the result of progressively combining all of the visible components from the bottom of the Component Tree, to the top. The resulting model is known as the Composite Model. The order in which components are combined can have a significant impact on the final shape of the composite model and so you will often need to move components relative to one another within the Component Tree in order to achieve the end result you are intending.

Watch this video to see this in action:

For more information, see the 3D Design and Management page.

To help you understand how the components are being combined, each component in the tree has an icon indicating how it is currently being combined with the components below

Add

Subtract

Merge

Low

Multiply

Group

Component Levels.

Every component exists on a single Level. These levels can be used to organize your modelling process. During the compositing process the contents of a level are combined first before the levels themselves are combined together.

Component Groups.

Grouped components are also indicated by their own icon and the presence of a plus or minus control to the left of the visibility checkbox. These controls allow you expand or collapse the group to show or hide the group contents, respectively.

Components can be selected in 3 ways:

• By left-clicking on the component's name in the Component Tree
• By left-clicking on the associated grayscale component preview image in the 2D view
• By double left-clicking directly on the component in the 3D view

In all cases, the new selection will subsequently be reflected in all three locations. So, for example, selecting a component in the Component Tree will simultaneously cause the associated 2D component preview to become selected in the 2D View, and the same component to become highlighted in red (or green if the selected component is obscured by another component) in the 3D View.

There are, however, some minor differences between the three methods of selection. Also, depending on the circumstances, there may be some advantages to selecting your components using one method rather than another.

The component tree works in a similar way to the Window's file explorer. To select a component, simply click on it. To select multiple components, hold down a Ctrl key while clicking on each component you wish to add to the selection. While in this mode, clicking on a component that is already selected will cause it to be removed from the selection.

Pressing a Shift key allows you to select a range of components. Click on the first component in the range to select it, then holding a Shift key and pressing the last component you want selected will select all the components between the first and last selection.

Double-clicking a component or level in the Component Tree will automatically open the Component Properties tool - see the Component Properties section for more information on how to use this tool to modify the selected components.

Right-clicking an unselected component in the Component Tree will select it, and open its pop-up menu of related commands. Any commands you select will apply to this selected component only.

Right-clicking a component that is already selected, and is also one of several selected components, will open a similar pop-up menu of commands. Any commands you select from this menu will apply to all of the currently selected components.

Because the left mouse button is used for twiddling the 3D view itself, a single left-click cannot be used for component selection directly. However, VCarve Pro's 3D view supports most of the standard selection concepts described above, using double-clicks instead. Therefore, to select a component in the 3D view it must be double-clicked with the left mouse button. To select multiple components in the 3D view, hold down a Shift key and double-click each of the components you wish to add to the selection. To access the pop-up menu of commands associated with a component, double right-click it in the 3D View.

Because components may overlap or merge through one another when forming the composite model, you may find that some components become difficult (or are even impossible) to select directly from the 3D view using the double click method. In this case you may use the right click menu. If you right click on a point above the component you wish to select then you are presented with a list of all the components that lie under this point.

You can also double right-click the selected component (highlighted in red) in the 3D view. The options offered include showing/hiding components, or setting their combine mode within the composite model.

In the 3D view selected object will often be tinted red. On some occasions parts of some components will be obscured by other components. In this case then the red tint will not be seen. The parts of the objects that are obscured will be tinted green so they are still visible from within the 3D view.

Many of the dynamic component editing tools can now be accessed directly from the 3D View. Editing the components in the 3D View makes it quick and easy to see the immediate effect of the changes to the Composite Model. To access these editing options a component or components must first be selected. Once selected then either clicking the component again in the 3D view or clicking the Transform Mode icon (Move, Scale, Rotate Selection) will activate the 3D Transform Handles.

The majority of these will function in the same way that they do with objects in the 2D View.

There are also icons below that can be selected that will allow you to edit the component properties in the 3D view.

Total Height

Shape Height

Base Height

Additional Settings

When selecting the additional settings option here you can adjust the Combine mode, Fade, Tilt and Appearance. When using the Fade and Tilt options in the 3D view you will need to set the direction of this in the 3D View instead.

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.

Watch this video to see this in action:

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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.

Watch this video to see this in action:

The quickest and simplest way to draw an ellipse is:

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

• Holding Alt and dragging creates an ellipse from the middle point.
• Holding Ctrl and dragging creates a circle.

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

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

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

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

Examples

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

To edit an existing ellipse:

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

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

VCarve Inlay toolpaths allow easy generation of the Pocket and Plug toolpaths to cut out your design in 2 Parts ready for creating a VCarve Inlay piece.

Once the toolpaths are generated, they will create 2 seperate toolpath sets, one for the Plug and another for the Inlay itself.

Both of these have their own slightly different Tool forms when editing them after an initial Calculation.

VCarve Inlay Toolpath - Plug

VCarve Inlay Toolpath - Pocket

Watch this video to see this in action:

This is the distance between the Top of the Plug and the Bottom of the Pocket when the 2 halves are placed together.

This value should be greater than 0 and less than the Pocket Depth.

0.001"~0.01" or 0.02~0.2mm are common values to use but can vary depending on your project.

This impacts the gap between the lowest point of the Plug and the highest point of the Pocket Material piece.

The Higher the Gap value the less material is left on the Plug to remove later.

The Smaller the Gap value, the closer the two material pieces will be and the more sturdy the Plug Piece will be.

A value larger the 0.0 and lower then the material thickness must be used.

Clicking the Select button opens the Tool Database from which the required VBit 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.

Check ✓ this option if you wish to use End Mill, Ball Nose or Engraving cutters to machine the large open regions of a design. If no tool is selected here but Flat Depth is specified then the selected V-Bit tool will be used to clear the flat areas as well as for the V-Inlay. All the tools in this section will leave an allowance for the V-Bit tool. Subject to this, the first tool in the list will remove as much material as it can, whereas subsequent tools will only machine areas the previous tools could not fit. The order of the tools in the list should match the order they will be run on the machine.

Clicking the Select button opens the Tool Database from which the required clearance tool can be selected and added to the list.

Clicking the Remove button will remove the selected tool from the list.

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.

Clicking the up and down arrow buttons will move the selected tool up and down the list respectively.

This allows you to select the Sheet the Plugs Vectors and toolpaths will be placed on.

If the same sheet as the original vector is selected then the Vectors and toolpaths will be placed mirrored from the original vectors position.

If a different sheet is selected then the new vectors and toolpaths will be mirrored and moved to the center of the new sheet.

If the final position of the new generated vectors needs to be adjusted, move the vectors as normal and recalculate all toolpaths to update the toolpaths to match.

Increasing the Boundary Offset will increase the material removed around the Plug.

Negative values will be ignored, you will only be able to use a positive values in this field.

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

Editing Modes

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

The three editing modes are:

• Vector Selection
• Node Editing
• Interactive Selection

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

This gadget is used to simplify the task of creating toolpaths to machine a rough blank to a finished diameter for users with a rotary axis / indexer. It supports rounding from either round or square stock and creates the toolpaths directly from the gadget. The gadget is designed to be used in a rotary job

As with all Vectric gadgets, the first part of the form gives an overview of the gadgets purpose.

The start of the form also makes a VERY important point about where the Z origin should be set when the toolpaths are output via a wrapping post-processor. This has to be configured during job setup.

You have the choice of specifying if the tool is being zeroed on the center of the cylinder or the surface. When you are rounding a blank, you cannot set the Z on the surface of the cylinder, as the surface it is referring to is the surface of the finished blank. We would strongly recommend for consistency and accuracy that you always choose 'Center of Cylinder' when outputting wrapped toolpaths as this should always remain constant irrespective of irregularities in the diameter of the piece you are machining or errors in getting your blank centered in your chuck.

A useful tip for doing this, is to accurately measure the distance between the center of your chuck and a convenient point such as the top of the chuck or part of your rotary axis mounting bracket. Write down this z-offset somewhere, and zero future tools at this point and enter your z-offset to get the position of the rotary axis center

The Create Rounding Toolpath form is divided into 4 logical sections.

If you are machining a square blank into a round shape, the previous options generate a large number of wasted toolpath moves, because for much of the machining process they are machining 'fresh air'. The 'Optimized Raster' strategy only creates the toolpaths where there is actually material on the blank and hence is much more efficient for square stock.

After choosing your machining method, the next section on the form allows you to pick the tool you will be machining with. The tool is selected from the standard Vectric tool database and will control the stepover, step down and feed rates for the toolpath. It is important to note that after choosing the tool you will not be able to edit the parameters, so you must set up the tool with the correct parameters in the tool database to begin with. This section also allows you to specify a name for the toolpath which will be created.

The values in the final section of the form are picked up automatically and are presented for reference only.

After filling in all the values (all values will be remembered as the default values to use the next time the gadget is run), press the OK button and the toolpath will be generated within the program.

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

One-time setup

Before we can begin, however, we must complete a couple of one-time steps to ensure your newly installed software is correctly configured. We will start by showing you how to log in to Vectric's online portal, V&Co. Here you will be able to download many other tutorials & projects, clipart packs and software updates. It is also the place you will find your personal product license code and you can return to it any time should you need to recover this licence information or use the main product installer again for any reason in the future. We will also use V&Co to access our online Machine Database. We can use this to automatically configure your software for the make and model of your CNC machine. Licensing and configuring your software typically only needs to be completed once and if you are online they can both be completed almost entirely automatically with just a few clicks.

Licence Management & Your V&Co Account

It is important that your investment in our high quality CNC software is protected and that Vectric can continue to create great software in the future - you will, therefore, have a unique personal licence for the software that you have purchased.

This licence is associated with your Vectric V&Co account, and can be accessed at anytime via https://portal.vectric.com. To log in to your V&Co account you will need to use the email address (which must be uniquely yours) and password that you registered with us when your account was created - please keep these details safe. Your registered email address is the way by which we can verify your ownership of the software.

Important Note: you can reset your password at any time using your registered email account and the forgotten password link provided on the V&Co log in page. If you need to change your registered email address it is important to do this before you lose access to the one to which the software is registered. If you can no longer access your registered email, you will need to contact us directly at support@vectric.com but please note that you will now need to be able to provide independent and alternative proof of your identity and purchase.

Within your V&Co account there is a unique digital code for each piece of Vectric software you have purchased. When you first run our software on your laptop or PC you will be prompted to provide this information. If you are installing onto a computer that is online (i.e. with unrestricted internet access available) you can complete this process almost entirely automatically - this is the fastest and easiest method.

The software will simply launch your web browser and prompt you to log in to your portal account. The software will then show the appropriate license that is available to be linked. Simply accept the link and you're good to go!

Once you have completed this process after initial install you will not be required to do it again unless you change computers or need to re-install the software afresh. Your software is now uniquely licenced to you and your details will always be shown in the main interface - even when you are offline, or online but not logged-in.

You can also log into your V&Co account from within the software at any time when you are connected to the internet to enable additional online features and services such as your clipart collection or online tool database.

When logged-in, your software will indicate this in the top right corner of the main window. Please note, the one-time licensing of your software and routinely logging in when using your software are independent concepts. Your personal product licensing is unaffected by your V&Co logged-in status.

We have also ensured that you can complete the software licensing process without having a live internet connection. The process is less automatic and details of the steps can be found here.

CNC Machine Tool Configuration

The software supports hundreds of different types of CNC machine, so the the next thing we will need to do is configure the software for your particular make and model. Correct configuration comprises two elements - appropriate tool settings in the tool database for your CNC machine and setting the 'translation' file (the Post-Processor) needed to create a toolpath file that your specific machine tool controller can understand.

Tool Database

Configuring the software will create a default tool database with tool definitions include cutter movement speeds ("feedrates") that *should* be a reasonable starting point for you to edit the entries for the tool types that you have, according to the recommendations from your CNC machine manufacturer for each material. Appropriate tool settings are the result of a complex interaction of the tool's shape and design, the nature of the material you intend to cut and the strength and power of your CNC machine. Don't use any default settings without first considering whether they are appropriate for your circumstances.

We will look at the Tool Database in more detail in the Toolpath Creation section below.

Post Processors

Your software can create toolpath files for hundreds of different CNC machines and controllers. To achieve this, the software creates an internal representation of a toolpath. Only when this toolpath is saved does it get 'translated' into the specific format required by your CNC machine.

The translation instructions are contained in file called a Post-Processor (because it *processes* the toolpath *after* it has been created).

Post-Processors also determing whether the toolpath movements will be presented to the machine using metric or imperial units. This must typically match the units mode you have set on your CNC machine's controller (seek advice from the manufacturer if needed). Note, however, it doesn't matter what units where used to create the original toolpath within the software - any required conversion is automatically applied when the toolpath is saved through the Post-Processor.

Job Setup - Axis Orientation

Our software is specifically designed for 3-axis CNC Machines (with additional support for an optional rotary axis). As you look at your CNC machine, the normal conventional is that left and right movement is controlled by the X-axis, forward and backward movement controlled by the Y-axis and up and down movement is controlled by the Z-axis.

In our software the width of your job will typically be equivalent to the X-axis of your CNC machine and the height of your job to its Y-axis.

Be aware that some machines are orientated so that the X & Y axes are swapped as you look at them - left to right movement may be controlled by the Y-axis and vice versa.

Use your machine's control software to jog your machine independently in each axis to make sure your expectations are correct.

Although unusual, it is possible that some post-processors will swap the X & Y toolpath coordinates after you have created your toolpaths - effectively changing the apparent orientation of you job - but this is only recommended for users who are confident of their machine's configuration and usage and not recommended for the majority of users who might not be aware of the other issues this can cause. Check with your machine tool manufacturer if you have any doubts.

It can help Orientate yourself so that when you stand before the machine, when you jog the machine to move to a higher X position, it is moving Left to Right infront of you. This can help visualise how the project design you have made in the software will translate to the bed of your machine.

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

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

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.

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

Watch this video to see this in action:

There are two choice of scaling mode:

• Scale selection
• Scale items individually

If scale selection is chosen then the whole selection is scaled as if it were a single group. If scale items individually is chosen then the scaling is applied to each of them as they were all selected one by one.

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

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

The keyboard shortcut T opens the Scale form in interactive mode

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

1. The Main Menu Bar (the Drop Down Menus) along the top of the screen (File, Edit, Model, Machine, Toolpaths, View, Gadgets, Help) provides access to most of the commands available in the software, grouped by function. Click on any of the choices to show a Drop-Down list of the available commands.
2. The Design Panel is on the left side of the screen. This is where the design tabs can be accessed and the icons within the tabs to create a design.
3. The Toolpath Tab is on the right side of the screen. The Top section of the toolpaths tab houses all of the icons to create, edit and preview toolpaths. The bottom half shows you toolpaths that you have already created.
4. The 2D Design window is where the design is drawn, edited and selected ready for machining. Designs can be imported or created directly in the software. This occupies the same area as the 3D View and the display can be toggled between the two using F2 and F3 or the tabs at the top of the window.
5. The 3D View is where the composite model, toolpaths and the toolpath preview are displayed, and can also be used to create your Vectors, 3D models and edit them both.
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.
7. Quick Drop down menus can be accessed here to change the current Layer, Sheet or Component Level you are working on.

The tool pages have Auto-Hide / Show behavior which allows them to automatically close when not being used, thus maximizing your working screen area.

The software includes two default layouts, one for designing and one for machining, which can automatically and conveniently set the appropriate auto-hide behavior for each of the tools pages. Toggle layout buttons on each of the tools pages allow you to switch the interface as your focus naturally shifts from the design stage to the toolpathing stage of your project.

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

Unpinned

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

In all three of the tools tabs there are 'Switch Layout' buttons. In the Drawing and Modeling tabs, these buttons will shift the interface's focus to toolpath tasks by 'pinning-out' the Toolpaths tools tab, and 'unpinning' the Drawing and Modeling tools tabs. In the toolpaths tab, the button reverses the layout - unpinning the toolpaths page, and pinning-out the Drawing and Modeling pages.You can toggle between these two modes using the F11 and F12 shortcut keys.

In all forms is a ? Icon which will take you to the appropriate Help Contents page to cover the tool form you are on in detail.

The Help Prompts will track your current tool or action and offer quick access to relevant Help documentation or tips on the current tool.

If you have downloaded a machine configuration and would like to edit it, or you would just like to create a new machine then you can do so from Machine Configuration Dialog.

This will allow you to edit, duplicate, add or remove machines. It will allow you edit the post-processor associations for each configuration.

1. Having a machine configuration allows you specifiy different feeds and speeds for your tools in the Tool Database.
2. And then it will allow you to easily select a machine to save your toolpaths with later on.

The Thread Milling Toolpath produces:

• internal thread, i.e., something you can screw a threaded bolt into.
• external threads, i.e., the threads for the exterior of a bolt.

It does this by using a special physical tool and a helical toolpath.

To use the toolpath select the vectors you wish to create threaded parts for. The center's of these vectors will be used to define the center of the threaded part.

Set the parameters to match the thread type you require, and then hit calculate to create the toolpath.

Watch this video to see this in action:

Clicking the Select button opens the Tool Database from which the required Tool can be selected.

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.

The thread milling toolpath supports two types of tool:

Single Point tools have a single point for cutting a single thread at a time

Multi-Point tools have multiple cutting teeth. They will cut all the threads with a single rotation

When using a single point tool then the created toolpath form a helix. The cutter at the side removes stock material to form the thread.

As seen in the above diagram, a single pointed thread mill tool is assumed to have a triangular cutting face. This triangle is the part of the tool that stands out from the shank of the tool and removes material:

The definition of the tool requires the following fields:

• S - The Tool Size. The horizontal size of the cutting part of the tool
• H - Tool Height. This is the vertical height of the widest part of the cutter face
• D - Tool Diameter. The diameter of the cutter measured from tip to tip.
• A - Tool Angle. The internal angle of the tool
• O - Tool Offset. This is the distance between the bottom of the tool and the tip of the cutter. It must always be bigger than the half of the tool size. Some tools may also have an additional offset, so it may exceed this value.

The Tool Height, Tool Size, and Tool Angle are all related fields. Changing one may change another. For example, if you modify the Tool Height, and the Tool Angle does not change, then the Tool Size must change. This change happens automatically when editing the tools within the tool databse.

It is possible to use a multi-pointed tool for thread milling. A multi-pointed has been designed to cut a single style of thread using a single helical motion. It will cut all the threads in a single go making it more efficient. However unlike single point tools it cannot cut different threads of different pitches.

In addition to the dimensions required for the single pointed tool, the multi-point tool also needs to know the threaded length. This is defined as the distance from peak to peak from the first cutting tooth to the last.

You can choose from one of a number of standard presets for the pitch. The standards are based on the ISO Metric Thread Standard for metric units, or the Universal Thread Standard for imperial units.

Selecting one of these options will pre-populate the pitch field with the correct value. If an external thread is selected it will also populate the fit tolerance field with a default value appropriate for the pitch. You are free to change this tolerance, however some tolerance will usually be required to have a smooth spinning thread.

Each thread has two diameters associated with it. These are the respective peaks and troughs of the thread.

The diameter on the form (sometimes referred to as the major diameter) is the largest diameter associated with the thread.

The fit tolerance controls how tight a fit the thread will have. Setting a positive tolerance will mean the tool cuts a slightly deeper thread.

In almost all practical uses, some form of fit tolerance would need to be applied in order to get a thread to run smoothly. Generally the fit tolerance is applied to the external thread but can be applied to both internal and external if needed.

There are two different types of thread it is possible to create:

• Internal Threads - These are threads for the female parts of connectors, e.g., nuts, threaded holes.
• External Threads - These are the threads for the male parts of connectors ,e.g. bolts.

The cut direction determines whether or not we want to machine the toolpath by sprialling downwards or upwards.

Which direction you choose will depend in some part on the relationship between the spindle direction, the tooling, and the desired finish.

The threads created by the Thread Milling toolpath are based around the ISO standard for threads. More information about this standard can be found here. This is based on tools with 60 degree angles and whilst we do not prevent other angles of tools from being used a 60 degree tool would give optimal results.

The result of using this standard is that the created threads will have flat regions as expected:

The Makerspace Connection Setup wizard guides you through the process of connecting your software with a specific makerspace. This wizard is designed to run once during the initial setup of the software and ensures a seamless integration between the two systems.

Before running the Makerspace Connection Setup wizard, make sure you have the following information and resources available:

• Access credentials to your V&Co account
• Administrator access to the organization which owns the copy of VCarve Pro Makerspace Edition
• Network connectivity to establish a connections with the server.

During the previous step, you may encounter an error message stating: "Too many machines are in use on this account. Please remove one to proceed." This error occurs when the maximum limit of 5 installations for VCarve Pro Makerspace edition has been reached. To proceed with the setup process, you need to revoke access for another device. Here's how:

1. In the error message, click the 'Manage Devices' button.
2. Your default web browser will open and redirect you to the V&Co website.
3. On the V&Co website, you will be prompted to choose a device to revoke access from.
4. Select the device that you no longer wish to have access to VCarve Pro Makerspace edition and confirm the revocation.
5. Once access has been successfully revoked, you can close the web browser and return to the software.
6. The setup process will automatically retry, and it should now complete successfully without the previous error.

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.

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.

Watch this video to see this in action:

The following shortcuts can be:

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

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.

Each layer in the list has five elements:

Status Icon

The leftmost icon indicates whether the layer is currently visible or hidden. Click on this icon to toggle the visibility of the layer.

The presence of a padlock shows that the layer is locked and cannot be accidentally edited.
Right-click the layer in the list and select the Unlock command to alter this.

Layer Colour

The color swatch can be used to color all the vectors on a layer. Click on the swatch icon Layer Color Icon and select a pre-set color from the color selector dialog, or choose 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. Layer Empty Content Icon a blank white sheet indicates that the layer does not currently contain any objects or vector geometry. If you import files from 3rd party CAD drawing packages via DXF or DWG format it is common for the file to include empty layers. This icon allows you to identify these empty layers and delete them.

Layer Name

To change the name of a layer, you can double click on this part of the layer item in the list to trigger in-situ editing. This works in the same way as file renaming in Windows Explorer. Alternatively you can right-click or use the layer's Pop-Up Menu icon to select the Rename command.

Pop-up Menu

Click the pop-up menu icon Pop-up Menu Icon for access to Activate, Lock, Insert, Delete and Merge layers as well as further ways to choose which layers to show and hide.

Select All on a Layer

Double-clicking on a layer in the Layers List will select all the objects on that layer. Alternatively you can choose the Select Layer Vectors command from the layer's pop-up menu.

Layer Ordering Arrows

Adjacent to the Layers List heading label are two arrow buttons. These move the selected layer up or down in the Layers List. This can be important to set the drawing order of objects that might otherwise obscure one another (specifically Bitmaps and 2D Component Previews). Objects on the top layers in the list are always drawn before objects in the lower layers and will, therefore, be 'underneath' them in the 2D View. You can use the Layer Ordering Arrows to resolve this issue.

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

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

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

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

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

Alternatively Gagdets can be assigned shortcuts.

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

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

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

• Celtic Weave Creator
• Dragknife Toolpath
• Keyhole Toolpath
• Setup Sheet Editor

Wrapping Sub-menu:

• Wrapped Fluting Layout
• Wrapped Spiral Layout
• Rounding Toolpath

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

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

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

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.

Watch this video to see this in action:

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

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

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

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

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

Example

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

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

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

Examples

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

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

This gadget simplifies the process of creating 'keyhole' toolpaths which are cut into the back of a sign or plaque to allow easy hanging on a wall. These slots are cut using a 'keyhole' cutter as shown on the left. The toolpath for these slots needs to plunge into the material at the mounting screw entry point to a depth that will ensure that the wide part of the cutter is below the material surface. The tool then moves along the 'slot', once it reaches the end of the slot, the tool retraces its path back along the slot to retract at the original plunge point.

Like all Vectric Gadgets, the top of the form gives brief instructions on how it should be used. For this gadget, you need to select one or more circular vectors in your design to indicate where you want the entry points for the keyhole slots to be before the Gadget is run. If you start the gadget without selecting one or more vectors to indicate these positions, the following warning will be displayed:

Once the form is displayed you can enter the parameters for your keyhole toolpath.

The data to be entered falls into three separate categories.

The final section of the form is used to specify a tool which the feed and plunge rates are picked up from, and also a name for the toolpath which will be created. As keyhole cutters are not supported natively by the program, just set up an end-mill with the required feed rates to use.

After entering all your parameters and pressing OK, the gadget will create a toolpath within the program to machine your slots and also the vector preview if you enabled this option. The screen shot below shows the preview vectors in the 2D view along with the toolpath in the 3D view.

This menu is displayed when you Right mouse click in 2D or 3D 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.

Many of these options are also Context Sensitive and will appear Greyed out when you right click something which cannot be targeted with that option.

This will bring up the following tool Box.

This slider will allow you to increase/decrease the amount of fading applied to this Bitmap/Component when it is not the currently selected item.

This can help if you want it to disappear into the background when working on other things, or to remain promanent and visible when working on other things. The default value for this is 50% and cen be set per item.

This will bring up the following tool Box.

This slider will allow you to increase/decrease the amount of fading applied to this Bitmap when it is not the currently selected item.

This can help if you want it to disappear into the background when working on other things, or to remain promanent and visible when working on other things. The default value for this is 50% and cen be set per item.

Remove From Curve:

If you have previously added your text to follow a curved Vector, this will allow you to remove it from that curve and return it to its original uncurved state.

Break Block into Lines:

If your text has more then one line of text in it, this will allow you to break that Text Objects into multiple text Objects, each made up of a Single line of the original Text.

Convert to Vectors:

This will convert a Text Object into a set of standard Vectors which can then be edited as normal vectors.

The Copy to and Move to options are unique to this Right click menu.

They have Level, Layer and Sheet modes, as well as Other Side which are Context sensitive, so will only show options which are applicable to the right clicked item.

• Copy to allows you to copy an object onto an existing Layer/Level/Sheet or to create a New one to copy it onto.
• Move to gives you the same choices but moves the original object rather than making a copy.
• Other Side copies the selected objects onto the other side in a two-sided job. The objects will be transformed so that they match up when looking through the material.
• Move to Front/Back is 2D View Exclusive and will bring items to the front or rear of other items on that same layer.
• Move to Up/Down is 3D Exclusive and will Raise or Lower the Components posiotion within its current Level.

If the current selection mode is set to Node Editing, one of two different menus will appear when the user clicks the RIGHT mouse button depending on whether the cursor is currently over a vector Node or a Span of a selected vector in the 2D View.

These menus have functions in them that correspond specifically to this selection and position. The menu shown here will appear when the cursor is over a Span of a vector in Node editing mode.

You can see a variety of choices:

• Convert the span to a Line, Bezier (curve) or Arc
• Insert a Point
• Cut the Vector at that point
• Delete the Span
• Insert a Midpoint
• Keep Bezier Tangency, which will fix the start and end directions of Bezier curves when they are being dragged directly, can be toggled on or off.

From this menu you can also Reverse the direction of the selected vectors, Close any selected open vectors, Join two selected open vectors or Exit node editing mode.

Many of these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the keyboard when the mouse is in position (over a node-edit vector span) instead of Right Clicking the mouse button to access the menu.

This menu will appear when the cursor is over a Node of a vector in Node editing mode.

You can see a variety of choices:

• Delete the Point
• Smooth it
• Insert a point at a virtual midpoint
• Cut the vector at that point
• Change the point to be the Start Point of the vector or extend the vector using the Polyline tool.
• Horizontal or vertical mirror mode for node editing can be toggled on or off.

From this menu you can also close any selected open vectors, Join two selected open vectors, Exit node editing mode or lastly see and edit the exact XY co-ordinate position of the node by selecting Properties.

Many of these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the keyboard when the mouse is in position (over a node-edit vector node) instead of Right Clicking the mouse button to access the menu.

When a Level in the Component Tree is selected and you RIGHT mouse click on it then the menu shown below will appear.

The first section allows you to make alterations to the selected level where you can change how the level combines with levels below it, you can choose to show or hide the level's visibility (and consequently the Components on it). Using the Select components option will select all the components within the level.

The next section contains the level effects which apply an effect to the level without affecting the individual components.

• The Clipping effect will dynamically clip the combined components on the level to the closed vectors which were selected when the effect was checked on.
• Mirror Mode allows you to mirror the combined components on the level in various ways.
• Wrapping is available for rotary jobs only and will allow components outside the job area that would otherwise be truncated to wrap around to the other side.

The next section allows you to insert new levels, delete the level and rename the selected level.

The final section of the menu allows you to export the complete contents of the level as a .3dClip file - when re-imported this would come into Aspire as a group.

This menu appears when a Component is selected in the Component Tree and you RIGHT mouse click on it:

The first option allows you to select the way the component combines with the other objects on its Level. You then have the option to position the components grayscale in the 2D View, by moving that to the Front or the Back. You then have the options to Copy and duplicate a component along with the option to Export the selected component as a .3dClip file. If you have more that one component selected you have the option to Group/Ungroup the components. You can delete and rename a component. There is also the option to show components, where you can choose to Show This, Show Only This, Show All But This and Show All. You can Hide a component, where an extra menu allows you to Hide This or Hide All. You can open the properties form for the selected component and the last option allows you to move the component to a new or existing Level within the Component Tree.

Import to Level

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.

Open Containing Folder

You can also the Folder which contains the clipart file in Windows.

Download

For clipart files included as part of the included clipart packs with the software, you will have the option to download them. See the Clipart guide .

Activate

Set this layer as the Active Layer.

Show

Select which Layers to show from a set of 4 options, and make them Visible in the Views.

Hide

Select which Layers to hide, and make invisible.

Lock

Lock this layer so that vectors on this layer cannot be selected.

Unlock

Unlock this layer so that vectors on it can be selected.

Insert New Layer

Create a new empty Layer, above the layer which was right clicked.

Delete

Delete this layer

Rename

Rename this Layer

Merge Visible

Collapse all Layers which are set to Visible currently, and place all Objects on those Layers onto this Layer.

Select Layer Vectors

Select all Vectors on this Layer in the View.

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

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

This toggles the visibility of the Toolpaths according to your choice. The next option allows you to Hide This or Hide All your toolpaths. Activate Sheet will make the sheet associated with the selected toolpath the active one.

You can Edit, Rename or Duplicate the selected toolpath.

The Recalculate submenu allows you to recalculate the selected toolpath, visible toolpaths or all toolpaths with any updated geometry selections.

Right mouse click > Recalculate will Recalculate the currently selected (highlighted) toolpath.

Right mouse click > Recalculate Visible will recalculate all visible (checked) toolpaths.

Right mouse click > Recalculate All will recalculate all toolpaths (across all sheets if there are multiple sheets within the current file).

Create an Empty Group will create an empty toolpath group which you can later place toolpaths inside. Group Visible will create a toolpath group containing the visible toolpaths.

Ungroup allows you to remove a toolpath group while preserving the toolpaths it contains. The Delete submenu allows you to delete one or more toolpaths, where you can Delete This, Delete All Invisible, Delete All Visible and Delete All.

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

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

Watch this video to see this in action:

Will retain any sharp corners in a design.

Offset with Sharp Corners on

Offset with Sharp Corners off

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.

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

This slider bar determines where the 3D model will be cut-off when converting to a Component. You can move this up and down with the mouse or use the Middle or Bottom buttons to locate the plane in the correct position.

If you are working in a 2 sided setup you can check ✓ this option and two components will be created - one looking down the Z axis from above to the zero plane and one looking up from below. Each side of the model will go onto a side. This will provide you with the geometry that can be edited to cut the original imported 3D part as a 2-sided job.

If you were importing a model that contains a non-convex surface for instance a bowl you can import the entire model on each side by sliding the slicing plane all the way to the bottom.

Checking ✓ this will help highlight any part of the 3D model which will lose detail when being imported by turning those parts of the 3D model Dark Purple in the 3D View.

As undercuts cannot be supported, any part of the model under this will be obscured and essencially lost once imported.

This tool will also highlight all parts of the model in Dark Purple which have Normal Issues in the original file. If you have large areas of the top surface of your 3D model highlighted like this and you do not get the import result you are expecting with your 3D model, you may need to investigate the original 3D model file in the original software used to create it to ensure it is solid and whole, and does not have parts of itself "inside out".

The final options are:

• Back will return you to the Import 3D Model > Transform form.
• Cancel will close the Import form and not import your model.
• Import with complete the process and convert your 3D model into a 3D Component within VCarve Pro

If you have recently purchased your machine which came with some licencse details for VCarve Pro (Registered User Name & License Code), you will have activated your software through the Manual License method from the License Dialog.

You have 90 days to register the software to obtain your own personalised license details through your own V&Co account.

In order to register, you just need to click Register Now... which will take you to a web page to register and create a V&Co account. This will allow you to retrieve your license details more easily and have access to our online features such tool database backup and online license entry.

If you are already registered, then you could just click Enter Personal License Details... which will take you the License Dialog.

If you click the Register Later button, you can continue to use your software but will be prompted again to complete the registration process.

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

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

Check out this video for an introduction to two sided machining:

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

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

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

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).

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

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

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

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

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

Watch this video to see this in action:

VCarve Pro has two smooth joining methods:

• A smoother method (new for V9.5)
• A more symmetrical shallower join method

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

Job sheets contain a summary of the information you will need when you come to run the toolpaths for your project at your CNC machine. Aspire will create a self-contained HTML document that can be viewed using most web browsers, including Internet Explorer, Chrome or Firefox. To create a job sheet for a given project, simply select Create Job Sheet from the Toolpaths menu and then select a filename and location to save the document. If your job contains multiple sheets, Aspire will automatically create a Job Sheet for every sheet that contains toolpaths. If you are working on a two sided job you will need to create a job sheet for both sides by simply switching between the sides and selecting the create job sheet icon, when you save the .html file the software will automatically add “_Top” or “_Bottom” to the name to differentiate between the two sides once the file has been saved.

Each job sheet document comprises the following information:

Job Layout

A thumbnail image representing the vectors on your current job / sheet, surrounded by an outer rectangle representing your material size.

Material Setup

A summary of the important pieces of information you will need to correctly position and datum your work piece at your CNC machine. This includes the dimensions of the material block used within Aspire to create and simulate your toolpaths. The home position from which your machine will start and return to. The clearance above the material for any rapid moves between plunges. For Two Sided Jobs you will also be displayed which side the setup sheet belongs to (top or bottom) along with the flip direction.

Toolpaths Summary

A summary of each of the toolpaths in the file, including the name of the toolpath, the tool required and an estimate of how long it will take to cut.

Toolpaths List

Details of each toolpath, including feed and plunge rates plus the intended spindle speed.

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.

Watch this video to see this in action:

Enter the diameter of the required circles

Selected Vectors

Circles Copied along curves

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

This will provide details of the changes that have been made between versions of this post-processor. This may be important for determining if you need to use an ealier or later version of a particular post-processor for your machine tool or controller.

This can be accessed from the Post-Processor list in the Machine Configuration Management dialog or the Post-Processor Management dialog.

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.

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 Selectordialog again (the settings are remembered) and uncheck the Associate with toolpath option.

If toolpaths with the Vector Selection mode set to Automatic are saved as templates, these setting are saved with the template. When the template is re-opened and the toolpaths recalculated, they will automatically select all vectors which match the filters specified with the Vector Selector for that toolpath.

If you load a toolpath template which has toolpaths associated with layers which don't exist in the current file, the Missing Layers for Template dialog will be displayed. It lists all the missing layers and offers you the choice of having them created automatically, deleting toolpaths associated with missing layers or just loading the toolpaths as is.

Choosing to allow the dialog to automatically create the missing layers allows a toolpath template to be used to create 'standard' layers for machining operations and load the toolpaths ready to be calculated. All you then need to do is move vectors to the appropriate layers and recalculate all the toolpaths.

Choosing the Delete all toolpaths associated with missing layers option allows you to create a single template with many toolpaths and have the ones which aren't appropriate to the current job automatically deleted.

The Toolpaths ► Templates ► Save All Visible Toolpaths as Template menu command (or the associated icon) allows a group of toolpaths to be saved as a single template. As an example, the toolpaths may have all the settings used for Profiling and Pocketing operations for a particular type of job and material combination. These toolpaths settings can then be recalled simply by opening the template and selecting the appropriate vectors for each toolpath.

If toolpaths with the Vector Selection mode set to Automatic are saved as templates, these setting are saved with the template. When the template is re-opened and the toolpaths recalculated, they will automatically select all vectors which match the filters specified with the Vector Selector for that toolpath.

If there are multiple sheets a message will be appear asking if you want to apply the template to every sheet in the job. If 'yes' is chosen the template will be applied to all the sheets and any toolpaths will be automatically calculated where possible. The toolpaths generated for each sheet will be prefixed by "Sn-" where 'n' is the number of the sheet for the toolpath. E.g if the template has a toolpath called "Cut Out" the associated toolpaths for each sheet will be:

"S1-Cut Out", "S2-Cut Out" etc.

If the template contains toolpaths that reference layers which do not exist in the current file the missing layers dialog will appear once and the option chosen will be used for every sheet the template is applied to. Choosing either 'Create the missing layers' or 'Load the toolpaths without creating missing layers' will mean that any toolpaths which reference those layers will be created as empty and have the visibility set to off.

If the toolpaths in the template use automatic vector selection then vectors matching the selection criteria can be created and the empty toolpath recalculated. If not using automatic selection an empty toolpath can be edited by double clicking on its name in the toolpath list or selecting the Edit Toolpath icon in the Toolpaths tab. Once the toolpath form is open, the vectors to be machined can be selected and the toolpath calculated using all the saved settings.

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.

When working in the 3D view additional icons will appear on the View Toolbar.

When you are working on a two-sided job additional icons will appear on the View Toolbar. 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.

The next icon indicates which side you are currently working on. This can also be clicked on to toggle between the single sided view or two sided view.

When you are working on a rotary job an additional icon will appear. This button allows you to toggle the 3D view between wrapped display mode and flat display mode.

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

Watch this video to see this in action:

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

This tool can be used in both the 2D and 3D View.

2D View offers a more direct way to view your vectors while 3D Offers more flexability to work with Vectors in 3D Designs and to make use of the Edit Boxes.

With this tool active, select 2 points across a 3D model to create a Vector of the 3D Components Cross Section.

Seen here is the Dashed Pink Cross Section Tool Line dragged over the 3D Component and the resulting Vector generated from it.

Watch this video to see this in action:

When Editing the Pocket part of a VCarve Inlay, you will be able to adjust the Start Depth (D) of the toolpath.

This will allow you to drop the Inlay toolpath into an existing Pocket you have cut in the project.

This can help if you are looking to add the Inlay into the bottom of a Bowl you have made for example.

This is fixed by the original VCarve Inlay Generation and is directly related to the Plug side of the toolpath.

If this requires altering, please delete both the Pocket and Plug toolpaths you have generated and remake them.

Prior to V11.0, we had the POST_BASE global variable as a way alleviating some of the repetitions inherent to post-processors to make their management and organisation easier. This seemed to create trouble over the years, so we have stopped supporting it.

This guide will help migrate from some of the old post-processors.

For the purpose of this guide, we will demonstrate this on the Next Wave post-processor, but the guidelines here can be applied to any post-processors.

In previous versions of the software then it was possible for a post-processor to have a base post-processor. The base post-processor had common sections in it. Then any other post-processor could take this post-processor as it's starting point, overwriting the bits it needed to. In this case we would say that this new post-processor inherited the base post-processor.

Assuming a post-processor Next_Wave_CNC_mm.pp which inherits the Next_Wave_CNC.pp post-processors:

The syntax of a typical POST_BASE statement is POST_BASE = "Next_Wave_CNC.pp"

Since this is no longer supported, we would need to replace this statement with the contents of Next_Wave_CNC.pp, removing any duplication from the copied content.

We have Next_Wave_CNC.pp (inch post-processor) with the content containing the following,

POST_NAME = "Next Wave CNC (inch)(*.tap)"

FILE_EXTENSION = "tap"

UNITS = "INCHES"

DIRECT_OUTPUT = ""

SUBSTITUTE = "({)}"

LASER_SUPPORT = "YES"

+------------------------------------------------
+ Line terminating characters
+------------------------------------------------

LINE_ENDING = "[13][10]"

+------------------------------------------------
+ Block numbering
+------------------------------------------------

LINE_NUMBER_START = 0
LINE_NUMBER_INCREMENT = 10
LINE_NUMBER_MAXIMUM = 999999

+================================================
+
+ Formating for variables
+
+================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR POWER = [P|A| S|1.0|10]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR CUT_RATE = [FC|A|F|1.1]
VAR PLUNGE_RATE = [FP|A|F|1.1]
VAR X_POSITION = [X|A| X|1.4]
VAR Y_POSITION = [Y|A| Y|1.4]
VAR Z_POSITION = [Z|A| Z|1.4]
VAR ARC_CENTRE_I_INC_POSITION = [I|A| I|1.4]
VAR ARC_CENTRE_J_INC_POSITION = [J|A| J|1.4]
VAR X_HOME_POSITION = [XH|A| X|1.4]
VAR Y_HOME_POSITION = [YH|A| Y|1.4]
VAR Z_HOME_POSITION = [ZH|A| Z|1.4]
VAR DWELL_TIME = [DWELL|A|P|1.2]
+================================================
+
+ Block definitions for toolpath output
+
+================================================

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"( [TP_FILENAME] )"
"( File created: [DATE] - [TIME])"
"( for Next Wave Automation from Vectric )"
"( Material Size)"
"( X= [XLENGTH], Y= [YLENGTH], Z= [ZLENGTH])"
"( Z Origin for Material = [Z_ORIGIN])"
"( XY Origin for Material = [XY_ORIGIN])"
"( XY Origin Position = X:[X_ORIGIN_POS], Y:[Y_ORIGIN_POS])"
"( Home Position)"
"( X = [XH] Y = [YH] Z = [ZH])"
"( Safe Z = [SAFEZ])"
"([FILE_NOTES])"
"(Toolpaths used in this file:)"
"([TOOLPATHS_OUTPUT])"
"(Tool used in this file: )"
"([TOOLS_USED])"
"([TOOLNAME])"
"(|---------------------------------------)"
"(| Toolpath:- '[TOOLPATH_NAME]' )"
"(|---------------------------------------)"
"G90"
"G20"
"[FC]"

We also have Next_Wave_CNC_mm.pp which inherits it as

POST_NAME = "Next Wave CNC (mm)(*.tap)"

POST_BASE = "Next_Wave_CNC.pp"

UNITS = "MM"

LASER_SUPPORT = "YES"

+================================================
+
+ Formating for variables
+
+================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR POWER = [P|A| S|1.0|10]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR CUT_RATE = [FC|A|F|1.1]
VAR PLUNGE_RATE = [FP|A|F|1.1]
VAR X_POSITION = [X|A| X|1.3]
VAR Y_POSITION = [Y|A| Y|1.3]
VAR Z_POSITION = [Z|A| Z|1.3]
VAR ARC_CENTRE_I_INC_POSITION = [I|A| I|1.3]
VAR ARC_CENTRE_J_INC_POSITION = [J|A| J|1.3]
VAR X_HOME_POSITION = [XH|A| X|1.3]
VAR Y_HOME_POSITION = [YH|A| Y|1.3]
VAR Z_HOME_POSITION = [ZH|A| Z|1.3]
VAR DWELL_TIME = [DWELL|A|P|1.2]
+================================================
+
+ Block definitions for toolpath output
+
+================================================

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"( [TP_FILENAME] )"
"( File created: [DATE] - [TIME])"
"( for Next Wave Automation from Vectric )"
"( Material Size)"
"( X= [XLENGTH], Y= [YLENGTH], Z= [ZLENGTH])"
"( Z Origin for Material = [Z_ORIGIN])"
"( XY Origin for Material = [XY_ORIGIN])"
"( XY Origin Position = X:[X_ORIGIN_POS], Y:[Y_ORIGIN_POS])"
"( Home Position)"
"( X = [XH] Y = [YH] Z = [ZH])"
"( Safe Z = [SAFEZ])"
"([FILE_NOTES])"
"(Toolpaths used in this file:)"
"([TOOLPATHS_OUTPUT])"
"(Tool used in this file: )"
"([TOOLS_USED])"
"([TOOLNAME])"
"(|---------------------------------------)"
"(| Toolpath:- '[TOOLPATH_NAME]' )"
"(|---------------------------------------)"
"G90"
"G21"
"[FC]"

We would like to change the contents of Next_Wave_CNC_mm.pp such that it does not have POST_BASE and does not depend on the content of Next_Wave_CNC.pp.

You will note that Next_Wave_CNC_mm.pp has changed the following,

1. POST_NAME
2. UNITS
3. LASER_SUPPORT
4. Various variables
5. The HEADER section

We have to ensure that those things are kept the same in the new Next_Wave_CNC_mm.pp.

This will serve as a rough set of steps on how to approach this.

1. Create a new empty file (called Next_Wave_CNC_mm_2.pp, for example) and copy the contents of the Next_Wave_CNC.pp into it.
2. Go through the old inheriting post-processor (Next_Wave_CNC_mm.pp) and copy / replace the variables and sections.
3. For example, replace POST_NAME, UNITS and LASER_SUPPORT

The beginnings of the new post-processor should look something like this

POST_NAME = "Next Wave CNC (mm)(*.tap)"

FILE_EXTENSION = "tap"

UNITS = "MM"

DIRECT_OUTPUT = ""

SUBSTITUTE = "({)}"

LASER_SUPPORT = "YES"

Keep going and replace / add the variables (starting with VAR).

Replace the begin HEADER section.

Diff the contents of Next_Wave_CNC.pp and Next_Wave_CNC_mm_2.pp and you should see that the differences are essentially the contents of Next_Wave_CNC_mm.pp.

Remove Next_Wave_CNC_mm.pp and rename Next_Wave_CNC_mm_2.pp to Next_Wave_CNC_mm.pp.

Cutting a Calibration Pattern

For our quick introduction we are going to us a 2D Profile toolpath strategy to engrave a precisely sized and aligned rectangle, circle and star. This pattern will use all the steps we have outlined in The CNC Workflow. It will also allow us to check that the CNC machine is working correctly using some simple but important features of the design:

• The rectangle, circle & star should not appear warped or distorted.
• The dimensions of the carved shapes should exactly match the design.
• The alignment points of the 3 shapes should not show any discrepancies.
• The star is rotated slightly clock-wise and the carving should match the original orientation of the design with no unexpected reflections in X or Y.

At the end of this guide we will review these checks and suggest some troubleshooting tips if any of them are not as they should be.

Material, Tooling & Hold-Down

The XY dimensions of the design will be 100mm (4") so you will need a piece of material approximately 150mm (6") square or larger.

The precise thickness of material is not too important as the design will simply be carved into its surface at a depth of 1.5mm (1/16"). Any piece that is 3mm (1/8") thick or greater will therefore be fine. An offcut of plywood or mdf board would be ideal.

To avoid any chance of collision with clamps or cutting into a screw, the best starting method to hold down a small piece of material like this is to use double sided tape. Any heavy duty 'carpet' type tape will work, but you may need to experiment to find a brand that secures well, but can also be cleanly removed once the job is complete.

The toolpth will be created based on a V-bit, but the precise tool angles are not important. If you don't have a V-bit tool, then a small (3mm, 1/8" diameter or less) end mill or ball nose tool will also work but the cuts will be the broader so the calibration pattern may be a little bit more difficult to interpret.

To avoid any chance of collision with clamps or cutting into a screw, the best starting method to hold down a small piece of material like this is to use double sided tape.

Create the Job

• Click `Create a new file` to get started.

This opens the `Job Setup` form. All projects start with a job setup. Here is where we consider the physical dimensions of our design. Note that you do not necessarily need to define the whole material block at this point, just that area needed for your design - the design area can be subsequently positioned anywhere on a larger physical material block using the `XY Datum Position`, which your CNC machine will use as its reference starting point.

Like all forms in the software, you should simply work from the top to the bottom of the `Job Setup` form. Forms are typically laid out with the most significant, non-optional or most commonly updated fields at the top. Sensible defaults are provided for most form fields the first time they are accessed (fields will generally remember their previous setting, once you edit them) so initially you can simply ignore any fields you are not sure about. At the bottom of most forms are the buttons to OK (accept), Apply or Cancel any changes you have made.

• The job setup form allows for projects that will be cut from both sides or using a rotary axis, but for now we will simply select `Single Sided`.

We will set the `Job Size` units according to your preference.

Note that your CNC machine controller will be set to expect toolpaths defined in either metric or imperial units and you will need to refer to your CNC manufacturer to determine your particular setting - the Post-Processor you select later will need to match the toolpath to the controller's requirements but this is entirely independent of the units you prefer for designing within the software - everything will be automatically converted, if necessary, when the toolpath file is created.

• Set the width & height of your new job to both be 150mm (6")
• Set the
• Click OK

Design the Calibration Artwork

Your project needs to start with design drawing. On the left-hand side of the screen there are a number of tabbed panels that provide access to various tools to help you to draw your design.

In due course, we will use our design to begin creating toolpaths for our CNC machine. The functions relating to toolpaths and toolpath strategies are located in another panel on the right-hand side of the screen. Initially this panel is hidden. Once our design is largely complete we will switch our focus to the toolpath panel on the right.

This is the typical workflow when creating a CNC project and so the software interface makes this switching of focus easy and intuitive.

For now let's continue to focus on the tools available in left-hand design panel.

The first thing we will do is create a simple 100mm Square, using the Rectangle tool in the Design Panel on the left. Witht he Rectangle tool open, click into the 3D View to place a default rectangle, and in the Edit Boxes on the Right and Bottom of the rectangle, click into each one and type 100.

This will create your Rectangle to be 100mm x 100mm.

Now press the F9 key on the keyboard, and your Rectangle Vector will now be centered in your work space.

Create our First Toolpaths

Now that our design drawing is complete we are ready to consider what toolpath strategy we should use to cut this shape accurately and efficiently.

The software interface can automatically hide the design tools panel and show the toolpath strategy tools panel using the 'Switch to Toolpath commands' button.

• Click on the 'Switch to Toolpath commands' button at the top of the 'Design' tab.

The toolpaths tab will now open on the right-hand side of the software. Here you will find all the tools relating to the creation, editing and saving of toolpaths.

Selecting the most appropriate toolpath strategy for a particular job is one of the toughest aspects of initially learning how to use your CNC effectively. Over time you will explore the different strategies available within this tab and our extensive tutorials and practical examples will to understand what each is used for.

For now we are going to use just the first strategy availble under the Toolpaths Operations - this is the Profile Toolpath.

Click on the Profile Toolpath button to open the 2D Profile Toolpath form.

Saving and Loading the Project

At this point we should probably save our project. Saving the project document using the File->Save menu, or the Ctrl+S shortcut-keys, is just like saving any other conventional application document (i.e. Microsoft Word etc.) and it will include all of your 2D design elements, 3D models and toolpath strategy settings in a `*.crv` or `*.crv3d` file. This is the file that you can come back to any time at a later date to continue your work or to duplicate as the basis of a new project.

Note that this is *not* the file that your CNC machine will read. Saving Toolpaths (see below) is the indepenendent process by which you specifically save the file from this project that your CNC machine needs. It may be helpful to think of the toolpath saving process as more like creating PDF files *from* your Word document - PDF files aren't typically reloaded or edited but they are ready for 'printing'.

Previewing the Toolpath

Before we begin getting our toolpath files over to our CNC machine there is still a *very* important step for us to do in the software. We can preview exactly how our CNC machine will move and what the material should look like after each toolpath is completed using the Preview Toolpaths command.

Saving Toolpaths - Post Processing

You now need to Post Process your Toolpath to save your toolpath out into a file which your CNC Machine will be able to read.

In this guide we will assume that you have completed the "Machine Configuration" Process either Manually or using one of the existing Online Configurations as seen here.

With that step complete, you just need to now open the "Save Toolpath" form, using the bottom right most icon in the Toolpath Panels icons.

Make sure your machine is currently selected in the Machine

Running Your Toolpath

Every CNC machine and controller is different. At this point you will need to refer to your CNC machine manufacturers instructions for the details of running your toolpath file, but we can provide some generally applicable information about the typical process you should expect.

Secure your material

Your piece of material will need to be secured to the machine's bed. This is typically done by clamping, screwing or gluing your material down (larger or more sophisticated machines may have vacuum hold-down). In the first two cases you must be very careful to avoid cutting into your clamps or screws. As we noted in the Job Setup, the toolpath file does not have to be the same size as the material so the simplest way to avoid clamps and screws is to make sure your job dimensions (and thus your toolpaths) are no larger then the unobstructed area of your material and that it is correctly positioned within this region.

Set your origins (datums)

The movements of all toolpaths are relative to the `XY datum position` you selected when you initially created your job (in our example we set the bottom-left corner, but it can also commonly be the center of your design), these are also often referred to as "origins". Now you must indicate to your CNC machine controller where this datum point is physically located on your material. This process is usually referred to as "setting the XY datum", "setting the XY origin" or "zeroing X & Y".

In effect, setting the XY datum will position where your toolpath will be cut on your material.