Move Selection
Selected items can be accurately moved and positioned using this option.
Anchor
The anchor position determines the point on your selected object's bounding box that will be moved to the absolute position entered.
Type of Move
Absolute
In this mode, the X Position and Y Position values will be used to position the object's anchor point directly
Relative
With this option selected, the values entered in the X Position and Y Position fields will incrementally offset the object from its current position, by the distances entered. The Anchor options are not relevant in this mode and so will be disabled.
The keyboard shortcut Mopens the Move form in interactive mode.
Edit Sheet - Single Sided
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.
In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a 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.
Job Type
Single Sided job type should be used when design only requires the material to be cut from one side. This is the simplest type of job to design and machine.
Double Sided Job type is useful when it is desired to cut both sides of your material. Aspire allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file.
Rotary job type enables the use of a rotary axis (also called a 4th axis or indexer).Aspire will provide alternative visualisation, simulation and tools appropriate for rotary designs.
Job Size
This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).
It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).
VCarve Desktop only supports job sizes up to a maximum of 25 inches square without tiling.
You can cut jobs larger than this limit but you will need to use the Toolpath Tiling feature to cut the job in sections.
Z-Zero Position
Indicates whether the tip of the tool is set off the surface of the material (as shown in the diagram) or off the bed / table of the machine for Z = 0.0.
XY Datum Position
This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's position.
Use Offset
This option allows the datum position to be set to a value other than X0, Y0.
Design Scaling
When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click
Modeling Resolution
This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.
As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.
The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.
As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.
Appearance
Clicking will pop up a dialog allowing you to set the color or material effect which will be applied to the base 3D model. It is possible to change this at any time and also to apply different colors and materials to different Components using the Component manager. See Preview Toolpaths to learn more about different material settings and adding custom material effects.
Tool Database
The Tool Database is used to make cutter management and selection very quick and easy, and reduces the possibility of programming jobs with incorrect cut depths and speeds and feeds. It allows pre-defined tools and settings (speeds, feeds, stepover etc.) to be selected from a list for a given machine / material.
The Tool Database can be accessed from the button through the various Toolpath forms. You can open the Toolpaths Tab button or through the Toolpaths menu.
Overview
This is a summary of the main entities and relationships in the database. More details on those will be given in the next sections.
- Tool geometry entities (organised hierarchically in the tree).
- List of Materials (Managed through the Material Management dialog).
- List of Machines (Managed through the Machine Management dialog).
- 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,
- Tool geometry: This is the physical properties of the tool such as the diameter, tip radius, etc...
- Cutting data: These include the Cutting Parameters and Feeds & Speeds of the tool. These values are defined for a particular material / machine.
Apply Changes
If you modify the Tool database, your changes will only be saved if you click OK. If you exit the Tool Database window using the Cancel button, any changes you have made since opening the Database will be discarded.
Tool Tree
The Tool Tree is located on the left-hand side of the Tool Database. Click on items in the list to see or edit their properties using the Tool Info section of the database window.
You can drag items up and down the list to change their order or drag them inside / outside of groups.
New Tool
Create a new tool with the default name for its type. The tool will be created with the first available type by default, but that can be changed through the Tool Type dropdown to the desired type.
Copy Tool
Duplicate the selected tool geometry or group in the list. If you're copying a tool, it will be copied without its cutting parameters.
The cutting parameters can be subsequently be:
- Copied from the same tool, different material.
- Tool with identical geometry, any material.
- Created with default values.
Delete Tool
Delete the tool as well as all of the cutting data for all machines / materials for which it was defined. If we're deleting a group, this will delete all the tools inside it in the same way.
New Tool Group
Create a new group in the tool database. Tools can then be dragged inside the newly created group. Alternatively, select the group and create a new tool directly under the selected group.
Export Tools
Export an individual tool or an entire group to a tool database file.
Import Tools
A tool database file can be imported into the currently open tool database. You will have 3 options,
- Import: This will simply import the given tools under the selected group (or as a top-level tool / group).
- Merge: This will attempt to merge the incoming tool group hierarchy with the current one (without any regards for selection)
- 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.
- Without overwriting: A new machine / material will be created to contain the cutting data of the incoming tools.
Tool Definition
When a tool or group is selected in the Tool List, its properties are displayed in the Tool Info section on the right-hand side of the Tool Database.
Name
This will go to the Name Format dialog to edit the name template for this tool type.
The name displayed here is then a result of evaluating the template in the current context (active machine, material and the cutting data defined for those as well as the tool geometry).
The name of a tool group can be defined directly through this dialog.
Tool Type
Various cutters can be specified in the database. Changing the cutter tool type is equivalent to creating a new tool, so all existing data for that tool (if any) may not be applicable anymore.
Notes
The tool notes section simply allows you to save any additional text descriptions, special instructions or relevant information you may require, within your tool definition.
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.
Diameter
The diameter of the tool in either inches or mm. The tool image will indicate where this dimension is taken from.
Number of Flutes
The number of Flutes for the bit. This is particularly useful if you would like to calculate a Chip Load value.
Cutting Data
The cutting data is the set of parameters which can differ between materials and machines. This set of parameters are defined to be per machine per material. The visible set of parameters are the ones for the active material / machine.
Creation / Copying
The cutting data is defined per material per machine. If the data is not defined already for a tool, we create it in a number of ways,
- Create with some default values which you can then change for your purposes.
- Copy from the same tool from a different material: This could be a sensible starting point if the materials have similar / close hardness.
- Copy from a different (identical) tool from the same (or different material)
Pass Depth
The maximum depth of cut the tool can cut. The Pass Depth controls the number of z level passes that are calculated for a toolpath.
For example, creating a pocket 1 inch (25.4 mm) deep using a tool that has a Pass Depth of 0.25 inches (6.35 mm) will result in the toolpath making 4 passes.
This value can be defined per machine / material depending on the machine's rigidity and the material's hardness.
Stepover
The distance the cutter moves over when doing area clearance cutting. For example, when raster machining the cutter will machine along the X axis, stepover in the Y direction and return parallel to the first line of cut. The greater the stepover the faster the job will be machined, but this must be balanced with the material being cut and the tooling being used, to ensure that the tool does not break. Therefore, this property (along with all other Cutting Parameters can be defined per material / machine).
When stepover's greater than 50% of the cutter / tip diameter are used the software automatically adds 'Tail' moves in the corner regions of toolpaths to ensure material is not left on the job for offset based strategies.
When using V-Bit Tools, the Stepover fields automatically change to use the following options.
Final Pass Stepover
The distance the cutter moves over when finish machining and is usually set to be a relatively small distance to produce a smooth surface finish on the job.
Clearance Pass Stepover
Only used when a V-Bit tool is being used to rough machine at multiple Z levels down to a specified flat depth. This stepover can be much larger than the Final Pass Stepover because the tool is only rough machining material away. Increasing the Clearance Pass Stepover will reduce the machining time, but you must be careful to ensure it is not too great for the material being cut.
Spindle Speed
Speed of tool rotation, specified in revolutions per minute.
Feed Rate
The surface cutting rate at which the cutter is moved in the material. The units can be specified in distance per second or minute.
Plunge Rate
The cutting rate at which the cutter is moved vertically into the material or during ramping moves. The units can be specified in distance per second or per minute.
Material / Machine
The Feed rate and Plunge rate you should use will vary depending upon the material being machined and the tooling being used.
Chip Load
This is the calculated Chip Load based on the entered values for the Number of Flutes, Spindle Speed and Feed Rate. This is displayed to conveniently be able to compare it with manufacturer-recommended Chip Load Values.
Maximum Burn Rate
This is the maximum speed at which the tool, when at 100% power, will still burn the material. This value is used for simulation purposes only. It should be calibrated to match your laser and material. A larger value will result in the simulated toolpath appearing darker.
You will need access to the Laser Module to create and simulate laser toolpaths.
Tool Number
This is the number of the tool needed to machine the job. When using a CNC machine with an Automatic Tool Changer (ATC), it is critical that the correct tool required to cut the job is located in the corresponding carousel location.
Per Machine
This parameter only needs to be defined per machine and so is shared between materials (unlike other cutting data parameters which are defined per machine per material).
Material / Machine Management
The cutting parameters / feeds & speeds section of the tool properties is defined for the active machine / material. This allows you to setup your tools with different values for each material or machine and switch between easily depending on the material you're going to use for the current job.
Material
The combo box is used to change active material. This can also be done by going to the Material Management dialog where materials can be added, removed or edited.
Machine
The combo box is used to change active machine. This can also be done by going to the Machine Management dialog where machines can be added, removed or edited.
Online Tool Database
The tool database can be stored and linked to your portal account so that it can be retrieved at any point from a different installation. For this, the software needs to be logged in to the portal account. Then, the database can be uploaded / download on request.
Login
Login to the portal to be able to access the currently stored tool database and / or upload your existing local one.
Download
Download the tool database stored on your portal account to replace your existing local tool database. This can be used for when we know there is a more up-to-date version online. You will also be prompted to update if that is the case.
Upload
When changes have been made to the tool database, this will upload it to the portal account so that it can be downloaded from any other location linked to the same portal account.
Remote Tool Database
Using the Right most Icon you can load a Remote Tool Database from a URL link supplied to you. More on this in the Remote Tool Database page.
Using Form Cutters
Form Cutters can be added to the Tool Database so that industry standard Ogee and Round-over type cutters, plus user definable custom shapes can be used for edge profiling and decorative carving.
Examples of these types of cutters and the kind of cuts they can be used for are shown in the images below:
Custom Form Cutters
Before opening the tool database, draw to exact scale the Right side of the cutter geometry in the 2D Window Use the Node Editing tools to create the arcs and curves etc.
Geometry
Only draw the Right-hand side of the cutter geometry to the correct size and scale as shown in the image above. The shape can be a combination of Lines, Arcs and Bezier spans.
Select the vector, then open the Tool Database dialog and create a new tool. Then, set its type to Form Tool.
The selected geometry will be imported and a profile displayed in the window. Give the Cutter a meaningful name. Enter the cutting parameters - speeds and feeds etc for the various materials you've got defined.
Click the Apply / OK button to save the new cutter into the database list so it can be used at any time.
Laser Module
Note
The Laser Module is available as a paid-for add-on to the software. The features are not included by default.
The Laser Module is a paid add-on for VCarve Desktop 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.
The Laser Cut - Fill Toolpath
Laser Cut - Fill Toolpath is used for cutting out shapes or marking areas.
Cut-outs can take into account the kerf, or width, of the laser beam to maintain the precise internal or external size the selected vector shapes. Shapes can also be filled with stripes or hatching to create simple shading effects.
The Laser Picture Toolpath
The Laser Picture toolpath uses the laser and through varying the power of the laser etches a copy of the selected bitmap onto the surface of your material.
Simulating Laser Toolpaths
Like all other toolpaths the laser toolpaths can be simulated. However, in the case of laser toolpaths, the simulation does not remove any material but instead marks the surface of the current simulation model. This marking is meant to simulate the charring of the material when scorched by the laser.
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.
Adapting a post-processor for Lasers
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.
Previous Post Processors will not work correctly with the Laser Module
Please note that many conversion kit manufacturers provided Vectric Post Processors before the release of the Laser Module. These used workarounds to allow some router toolpath strategies, such as profiling, to be used with a laser head. Post Processors created without explicit support for the additional features documented here will not work correctly.
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 onJET_TOOL_POWER
- Output whenever the toolpath needs the laser power to changeJET_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
SketchUp files with a .SKP extension (see www.sketchup.com) can be imported as 2D data suitable for machining into a VCarve Desktop job using the File ► Import Vectors... command from the menu bar or the import vectors icon on the Drawing tab. To import data from a SketchUp file you must already have created or opened a job to import the data into.
As a SketchUp model is usually a 3D representation of the part, the SketchUp importer offers a number of options to allow you to start manufacturing the model.
We will illustrate the two main choices for how the model will be imported using the SketchUp model shown to the left.
The model shown in the screenshots is a cabinet constructed by following the instructions in the Fine Woodworking 'Google SketchUp guide for Woodworkers: The Basics' DVD which is available via the Fine Woodworking site at www.finewoodworking.com. Vectric have no affiliation with Fine Woodworking, we are just using screenshots of the model constructed while following their tutorials to illustrate the process of importing a SketchUp model.
Layout of Imported Data
In the first section there are two main choices for how the data from the model will be imported, 'Exploded Flat Layout' and 'Three Views - Front, Top, Side' as shown below.
Exploded Flat Layout
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 Desktopcan be used to layout the parts with more control and across multiple sheets
Three Views - Front, Top, Side
This option will create an 'engineering drawing' style layout of the SketchUp model as shown in the screenshot below.
The size of the model is preserved and it is relatively simple to pick up dimensions for parts you are going to manufacture from the various views. The colors of the lines you see are taken from the colors of the original SketchUp layers the various parts of the model are on.
Create Circles / Arcs
SketchUp does not maintain true arc or circle information for the boundaries of its parts. This is a problem when it comes to machining as the 'polygonal' SketchUp representation can give very poor machining results. For this reason, VCarve Desktop offers the option to refit circles and arcs to imported data.
The screenshot above left shows the results of importing a part with a filleted corner and hole with these options unchecked. The 'fillet' is made up of a series of straight line segments and the circular 'hole' is actually a polygon made up of straight lines.
The screen shot above right shows the same part imported with both these options checked ✓. The 'fillet' now consists of a single smooth arc and the circular 'hole' now also consists of arcs rather than straight line segments. Both these features will machine more cleanly in this form.
Data to Import
A SketchUp model will often contain parts that you do not wish to machine (such as hinges, knobs etc.) or data which will be cut from different thicknesses of material and hence different parts need to be imported into different VCarve Desktop jobs. To allow control over what is imported you can choose to only import parts of the model which are on particular layers using this section of the dialog.
To only import data from selected layers, choose the 'import visible data on selected layers' option and click the check box next to each layer to indicate if you want to import data from that layer. Note that the number of parts on each layer is displayed next to the layer name.
It is very easy to assign different parts of the model to different layers within SketchUp to help with the import process into VCarve Desktop. The screenshot below shows the result of only importing data on the 'Door' layer from the example.
Component / Group Handling
This section of the form allows advanced handling of how 'parts' within the SketchUp model are identified and treated on import.
Group imported parts
This option is normally selected for all but the simplest models as it allows each 'part' of the model to be selected, moved and nested easily after import. You will need to ungroup the imported data after nesting etc. to allow individual features to be machined. By default, VCarve Desktop will treat each SketchUp group / component as a single part UNLESS it contains other groups or components within it, in which case each lowest level group / component will be treated as a separate part.
Items which you retain in groups can be ungrouped at any time in the usual ways.
If the right-click menu-option to Ungroup back onto original object layers is used (which is the default option when using the icon or shortcut U) then the software will place the ungrouped items back onto the original layers they were created on in SketchUp.
Keep components starting with two underscores (__) together
If you have a complex model which contain 'parts' which are made up of other groups / components, you will need to do some work on your model to identify these parts for VCarve Desktop. The way this is done is by setting the name of the groups / components that you wish to be treated as a single part to start with__ (two underscore characters). For example, if you had a model of a car and you wanted the wheels / tires / hub nuts to be treated as a single part even though the Tire, Wheel and other parts were separate components, you would group the parts together and name them something like __WheelAssembly in SketchUp. When this model was imported, and VCarve Desktop reached the group/component with a name starting with __ it would treat all subsequent child objects of that object as being the same part.
Replace outer boundary (for flat jobs only!)
There is a style of 'building' with SketchUp where individual 'parts' are made up of several components 'butted' against each other. The screenshot below shows such a component.
This object is made up of many smaller components representing the tabs on the top, the connectors at the end and the support at the bottom as shown below.
Although when can treat this as a single 'part' when imported by starting its name with __ (two underscores), the imported part is still going to be difficult to machine. The screenshot below shows the part imported into VCarve Desktop without the 'Replace outer boundary' option checked ✓. The part in the image has been ungrouped and the central vector selected.
As you can see, the outer boundary is made up of separate segments for each 'feature'. VCarve Desktop does have the ability to create an outer boundary for vectors but this can be time consuming if it has to be done manually. If the 'Replace outer boundary' option is checked, ✓ for every part VCarve Desktop will try to create a single outer boundary and delete all the vectors which were part of this boundary. The screenshot below shows the result of importing the same data with this option checked, ✓ this time the part has been ungrouped and the outer vector selected.
This data is now ready to be machined directly. It is important to understand the limitations of this option. It can be substantially slower. Creating robust boundaries for each part can consume a lot of processing power. Any feature which shares an edge with the boundary will be deleted. If the tabs on the top of this part were to have been machined 'thinner', this approach would not have been suitable as the bottom edge of the tabs has been removed.
IMPORTANT
The new features will help a lot of SketchUp users dramatically reduce the time it takes to go from a SketchUp design to a machinable part using Vectric Software. It is important to understand though that while these options provide a useful set of tools, in many cases there will still be additional editing required to ensure the part is ready to toolpath. Understanding the options and how they work will allow the part to be designed in SketchUp with these in mind and therefore help to minimize the time to machine once the data is imported.
Note
Sketchup files will only open in the same bit version you are running e.g. A file saved in a 32 bit version of Sketchup will only open up in a 32 bit version of the software.
Moulding Toolpath
This icon opens up the Moulding Toolpath Form. This form is used to create a toolpath from a drive
rail and a profile. The result of machining the toolpath is the extrusion of the selected cross-section profile along the pre-selected drive rail. Although strictly speaking the result of this is a 3D shape because it does not use a 3D model it is classified as a 2.5D Toolpath.
Toolpath Position
You now need to determine the toolpath position within the material. The Z Height of the toolpath is determined by the height of the selected cross section. You can interactively position the toolpath by pulling on the slider or you can enter exact values in the edit boxes.
Note
If the cross section you have selected is higher than the material thickness then you will need to change your material thickness in the material setup form to accommodate the profile height, or exit the form and edit the height of the cross section vector you are using to create the Moulding Toolpath to fit within the material block.
Drive Rail Selection
From the 2D view, select the drive rails for the toolpath followed by the profile you wish to extrude.You may select multiple rails.The last selected vector is the Profile that you are extruding.
In the 2D view your rail vector will now be colored orange and will show a green square indicating the start point, along with arrows along the vector showing you the direction.
The direction and start point may not be what you intended, you can change the direction (and start point location on an open vector) by right clicking in the 2D View on the vector and choosing .
The button on the form can be used at any time to empty your current selection; this will deselect the drive rail and if already selected the cross section too. This can be used if you want to change the selection without exiting the form.
Cross Section Selection
After you have chosen your drive rail the next step is to select a cross section that will be swept around the drive rail to create the moulding. The cross section needs to be an open shape in order for this to work.
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.
Note
On a closed vector shape, the cross section profile will always hang on the outside of the shape. Therefore, your drive rail vector should always represent the inside edge of the border/frame shape for which you are creating the toolpath. To change the direction in which the toolpath is created, click the Reverse Rail option on a closed vector drive rail.
Selecting a Tool
The next step in this form is to select a tool to finish-cut the moulding shape. This would typically be a ball-nose or tapered ball-nose tool but that may vary depending on the shape you plan to cut. To select a tool use the button to access the Tool Data Base. If the tool you require is already shown as the selected tool, you can use the Edit option to check and/or modify the tool settings for this particular toolpath.
Note
The generated toolpath will follow the shape and direction of drive rail vector. At the end of an open vector it will lift by at least the stepover distance, step over and then come down to the surface again, returning along the vector in the opposite direction, this small lift is designed to avoid leaving connecting marks on the surface of the part and so improve the potential finish quality. On a closed vector after completing a pass the length of the vector it will lift, step-over, return the tool to the profile shape and continue cutting in the same direction - this direction can be reversed by right clicking the drive rail vector and using the Revers Rail option to change the direction of the arrows on the vector.
Vary Stepover
Typically the Stepover value specifies the horizontal distance that the tool will step over and this is projected onto the 3D model. Checking ✓ the Vary Step Over option will instead adjust the step over based on the shape of the cross section profile vector rather than just projecting the standard pattern down Z. In cases where there are steeply curved, angled or near vertical edges this should result in passes that are closer together, in most situations this will improve the finish quality but also potentially increase the machining time
Skip Flat Regions
This choice will only become available when the option is checked ✓ to Machine Flat Regions when using the Larger Area Clearance Tool in the next section of the form. When this is active the software will look to identify flat areas of the cross section profile that can be machined with the larger tool. If these regions are detected and Skip Flat Regionsis also checked ✓ then the finish tool will avoid re-machining those flat areas as in most cases they should already have been completely finished by the Larger Area Clearance Toolpath.
Use Larger Area Clearance Tool
If this option is selected, then two tools are used to cut the shape. In effect the Larger Area Clearance Tool is similar to a 3D Z Level Roughing toolpath and would be cut first. It will use the tool parameters to generate multiple depth 2D pockets following the direction of the selected rail to clear away excess material. This should be used if the material is too deep and/or hard to cut directly with your selected finishing tool. As documented above and below using this option with a flat shaped tool can also be very beneficial to the machining time and finish on cross section profile shapes with flat/horizontal regions.
When you use the option to Use Larger Area Clearance Tool, the software will calculate two toolpaths, the first will have [Clear] in its name to differentiate the two, [Clear] being the toolpath associated with the Use Larger Area Clearance Tooland the other, is the finish toolpath using the smaller tool. The [Clear] toolpath should be run first on the machine:
Machine Flat Regions
If this option is checked ✓ then the software will try to detect flat/horizontal areas in the cross section profile. If the specified Larger Area Clearance Tool can fit into these areas then they will be machined as part of the roughing operation. When using a flat tool this should give both a superior finish and also help to reduce the cutting time. Having this option checked ✓ will also allow you to choose the option Skip Flat Regions in the finish tool section which will stop the secondary toolpath from re-cutting these areas.
Note
This option will override the Machining Allowance value in the flat areas of the shape to ensure they are machined to the correct depth and not left with additional material on.
Ramp Plunge Moves
The Larger Area Clearance Tool can be ramped over the specified distance instead of plunging vertically into the part. For some tool types and shapes, this approach can reduce the heat build-up that may damage the cutter and also reduces the load on the spindle and z axis bearings.
Machining Allowance
The machining allowance is a virtual thickness which is added to the moulding profile when the Use Large Area Clearance Tool is calculated. This ensures that the toolpath leaves some extra material on the part cut with a larger tool.
Note
If you have the option selected to Machine Flat Regions the Machining Allowance will only be applied to the other areas of the cross section profile, on the detected flat regions the software will cut down to the actual surface and ignore the Machining Allowance value within those areas ensuring that they are cut to the thickness specified by the cross section profile vector.
Create Sharp Corners
This option can be checked ✓ when working with rails that have sharp corners, allowing you to force the software to try and emulate these in the Moulding toolpath. Below you can see the effect of checking ✓ this option on a closed vector shape with the standard corners option on the left showing the toolpath rolling around the shape edge and the Sharp Corners option on the left where it has forced mitre style corners in the machined shape.
Boundary Offset
This option can be used to force the toolpath to cut past the edge of the part that is parallel to the drive curve vector. By default the center of the tool will go to the edge of the ends of the selected profile vector as its extruded along the drive rail. It may be desirable to extend this distance to either force the tool down the edge of the profile shape with vertical or steep edges or to ensure the toolpath has gone far enough past the edge to cleanly cutout the final shape with a profile toolpath. The value entered for the Boundary Offset will force the tool past the ends by the specified amount. As such if you want to ensure a vertical or very steep edge at your profile ends is machined you will need to specify a value which is at least the radius of your tool plus a small additional amount (say an additional 10% of the radius). For example if you are using a 0.25 inch (6mm) diameter ball-nose tool for the finish cut then you would specify a minimum of 0.15 inch or 3.6mm (= tool radius + 10%) to ensure the tool would be forced down the edges of your shape. If you wanted to ensure the roughing had also been able to machine these areas then the value should be based on your Larger Area Clearance Tool size instead.
Use automatic boundary offset
When this option is selected, VCarve Desktop will calculate the boundary offset to ensure that the tool fully cuts the ends of profile, even if profile ends in vertical/steep edges.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Automatic Vector Selection
Like many of the other toolpaths the Moulding toolpath can use an automatic vector selector (see here for more details). In the case of the Moulding toolpath there are two separate selectors, one for the rail and one for the profile. Both work as any other selector does and will be saved with any toolpath template that uses them.
V-Carve Toolpath
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.
Cutting Depths
Start Depth (D) specifies the depth at which the V-Carving toolpath is calculated, allowing V-Carving / Engraving to be machined inside a pocket region. When cutting directly into the surface of a job the Start Depth will usually be 0.0. If the V-Carving / engraving is going to be machined into the bottom of a pocket or stepped region, the depth of the pocket / step must be entered. For example, to carve or engrave into the bottom of a 0.5 inch deep pocket, the Start Depth = 0.5 inches
Start Depth (D)
Start Depth (D) specifies the depth at which the V-Carving toolpath is calculated, allowing V-Carving / Engraving to be machined inside a pocket region. When cutting directly into the surface of a job the Start Depth will usually be 0.0. If the V-Carving / engraving is going to be machined into the bottom of a pocket or stepped region, the depth of the pocket / step must be entered. For example, to carve or engrave into the bottom of a 0.5 inch deep pocket, the Start Depth = 0.5 inches
Flat Depth (F)
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
Tool
Clicking the 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 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.
Use Clearance Tools
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 button opens the Tool Database from which the required clearance tool can be selected and added to the list.
Clicking the button will remove the selected tool from the list.
Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database.
Clicking the up and down arrow buttons will move the selected tool up and down the list respectively.
Clearance Tool Options
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.
Use Vector Start Points
If this option is checked ✓, the start point of the profile and offset toolpath segments will be as close as possible to the start point of the corresponding boundary vector. Otherwise this is left up to the program.
Use Vector Selection Order
If this option is checked ✓, the vectors will be machined in the order you selected them. If the option is not checked the program will optimize the order to reduce machining time.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Project toolpath onto 3D Model
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.
Note:
When a toolpath is projected onto the 3D model, its depth is limited so that it does not exceed the bottom of the material.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Join Open Vectors
The icons to join and close vectors are located under the Edit Vectors section of the Drawing Tab.
Open vectors are automatically identified and closed or joined to other vectors where the end points lie within the user definable tolerance.
Distort Object
This tool allows you to bend and flex a vector or component by manipulating a distortion envelope using standard node editing tools. You can select one or more vectors or components and then use one of the three different tool modes to create your initial distortion envelope.
Multiple Objects
You can distort several vectors or components at once but you cannot distort a mixture of vectors and components together in a single operation.
Once the distortion envelope has been created, you can use the node editing tools to add or edit its nodes and spans. As you alter the shape of the envelope the associated object will be distorted to reflect the changes.
Layers
When distorting a selection of objects which fall on different layers, the result will be created on the layer of the first object in the selection.
Use Rotated Bounds
This option is only supported if you only have one object selected to distort. It makes use of the local rotation of the object as shown in the Selection Tool.
When this option is ticked,
- The initial distortion envelope is created along the transformed bounds of the selected object.
- When distorting along a curve (or two), the object is distorted on the curve in its local transformation. This is useful if you're distorting a rotated object onto a rotated curve, for example.
Bounding Box Distortion
This option is available if you have a selection of vectors or components (Note that you cannot mix vectors and components in this mode). It creates a distortion envelope based on the closest bounding box that can be drawn around your selection. Thus the resulting envelope is always initially a rectangle, comprising four line spans and a node at each corner. Using the normal node editing tools, however, you can modify this envelope as much as you like and the shape within it will be distorted accordingly.
Along a Single Curve
This option is only available if the last item in your selection is an open vector that can be used to define a curve, above which the other selected objects will be distorted. The distorted object can comprise one or more vectors or one or more components, but not both.
Using this option, you will usually end up with your objects bent to match the curve in your original selection. The distortion curve itself is left unchanged by this operation.
Between Two Curves
This option will become available if the last two objects in the current selection are open vectors, between which the other objects can be distorted.
Baking Distortion into an Object
Once an object has been distorted, node editing will always relate to the object's distortion envelope. If you wish to edit a distorted vector directly again, you will first need to permanently apply the distortion to the shape.
If you select an object that already has a distortion envelope while in the Distort Object tool, the button will be available. Clicking this button will permanently apply your current distortion and you will then be able to either distort the object again (with new settings), or node edit the shape directly.
Baking Components
If you try to use this tool to modify multiple, grouped or distorted components you will first be prompted to 'bake' your selection components into a single object. For more information on what this means, please see the section Baking Components.
Redo Operation
Clicking this option steps forward through design steps that have been Undone using the Undo command (see above) to get back to stage that the user started using the Undo function.
Text Selection
The Text Selection tool allows the user to adjust kerning, line spacing and bending the text on an arc. The text will be displayed as magenta lines with 2 Green handles in the middle for arching the text.
If the selected text was placed on a curve the handles will not appear, as such text cannot be arched.
Letter Kerning
The interactive kerning and line spacing cursor is shown when placed between letters or lines:
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
Line spacing can be modified by placing the Edit Text cursor between lines. It will change to the line spacing cursor:
Clicking Left mouse button will move the adjacent lines of text closer together.
Holding the Shift key and clicking the Left mouse button will move the lines apart.
Holding the Ctrl key doubles the distance each line moves on each mouse click.
Holding the Shift and Ctrl keys together and clicking the Left mouse button moves the lines apart in larger increments.
Text Arching
The interactive rotation and movement cursor is displayed when the cursor is placed over either of the Green Handles to indicate that the text can be arced either Upwards or Downwards:
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.
Moving
There are two white handles for moving the text, one in the middle of the text, and one in the center of the arc, though that may be off-screen for very shallow arcs.
Rotating
Clicking and dragging the Red boxes rotates the text around the center point of the arc.
Holding the Ctrl key forces the rotation to be in 15° increments. This allows the text to be positioned exactly on the horizontal or vertical quadrants, even after it may have been moved slightly.
Changing arc radius
Clicking and dragging the Blue boxes changes the radius without moving the arc center.
Circular Copy
This tool will automatically create a repeating pattern by making copies of the selected object and positioning them around a full or partial circle. The number of copies to be made can be entered directly.
Selected Objects Size
Reports the current size of the selection that you are intending to copy. This is for information only, but the values can be selected, copied and pasted to use in other calculations.
Rotation Center
This is the absolute XY coordinate around which the objects will be rotated when copied and pasted. The default Rotation point is the middle of the selection. You can set the rotation center coordinates explicitly using the X and Y edit boxes on this form or by clicking the selected geometry to show the transform grips, then double-clicking the center one to show the pivot-point and dragging the Pivot Point handle associated with the selection in the 2D View:
Rotate Copies
This option controls whether the copied objects are each rotated as they are placed around the circle, as shown in the diagrams below. If this option is selected, each copy is rotated according to its position on the circle. If the option is not selected then each copy maintains the orientation of the originally selected object.
Angle
Total Angle
With this option selected the number of items is divided into the Total Angle to give the incremental angle between each object.
Step Angle
With this option selected this angle is used to copy the selected vector(s) by this angle x the number of Items.
Note
A negative step angle pastes the copies in a counter-clockwise direction. A positive step angle pastes in a clockwise direction.
Preview Toolpaths
Calculated toolpaths can be previewed to see exactly what they will produce when cut into the material. The 3D preview mode also allows the job to be viewed in different material types with the option to paint the machined regions with a Fill Color.
Active Sheet
The active sheet label shows the sheet that is currently active. Each sheet can be given different material settings. The active sheet can be toggled by clicking within the 2D view, or using the dropdown menu in the toolpaths tree.
Material Selection
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.
Use Solid Color
If this is selected the color for the material can be selected from the color picker below the list.
Use Material
The user can choose from the list of pre-defined material effects by clicking on appropriate position on the list. These include many wood grains, metal effects, stone and plastic.
Adding Custom Materials
Additional materials can be added to the library using the list itself. You can add a category (folder) which groups your textures using <Create 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.
Machined Area Color
Material Color
With this setting, the areas of your preview will simply be colored using the material defined above. Effectively this switches off independent material settings for your machined areas.
Global Fill Color
Paints all the machined regions with the selected color. Selecting the associated pull-down list opens the default color selection form. Click on one of the preset colors, or click to create a completely custom color.
Toolpath Color
If this option is selected, each toolpath can have a different color assigned. If the 'No Fill' option is selected from the color picker form, the current toolpath will be shown in the material color.
Choose the color you want for the fill of that toolpath and it will be applied to the areas that the toolpath has carved when they are previewed. Once you assign an individual color a small square of that color will be displayed next to the name in the toolpath list. This can be seen top left of each tool icon:
Lithophane
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.
Animation Settings
Animate preview
This option will show the material being removed by the cutter as the preview is drawn.
Draw tool
This option will show a wireframe animation of the tool (to scale) cutting the job.
Toolpath Preview Tools
Preview Toolpath
This option animates the selected toolpath cutting into the material
Preview Control Simulation
The preview controls provide full video-like playback control of your toolpath. You can use this mode to analyze the tool moves in detail, step-by-step. To begin using Preview Control, click on either the Run, Single Step or Run to Retract buttons
Preview All Sides
This option animates all calculated toolpaths cutting into the material on both sides if working in a two sided environment without being in the 'Multi Sided View' mode (This option will be grayed out if working in a single sided setup)
Preview All Toolpaths
This option animates all calculated toolpaths cutting into the material
Preview Visible Toolpaths
Previews all the visible toolpaths
Reset Preview
Resets the material back to a solid block
Save Preview Image
Saves an image of the 3D window as a BMP, PNG, JPG or GIF file
Slice Model
The slicing feature allows the user to divide the Composite Model into Z-Slices each of which will become a Component. This is for customers who need to cut a part which exceeds the Z depth of their machine gantry, the cutting length of their tools or the thickness of the material they are using. Once the slices have been cut on the CNC then they can be re-assembled to make the finished full depth part.
When this function is executed each slice will become a Component in the Component Tree and can then be moved into position and have toolpaths calculated on it. An example of this is shown in the images below, on the left it shows a scallop shell component that is 3 inches thick, the image below right shows this divided into two separate components, each a 1.5 inch slice of the original.
Note
Before using the Slice model command it is important to make sure that you hide any components that you do not wish to include in the operation.
When the icon is clicked the Slice Model form will appear. This can be used to control the number and thickness of slices which will be created. At the top of the form it will display some reference information showing the thickness of the current Composite Model and also the currently defined Material Thickness (for machining).
Model Slicing
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.
Slice Thickness
Checking this option allows you to specify the default slice thickness. You can choose if you want to slice from the top down or bottom up using the From Top checkbox. Each slice is will be the specified thickness, except for the final slice which will be whatever height remains after all the other slices have been taken. If From Top is checked then the final and potenitally thinner slice will be at the bottom. If From Top is uncheched then the final and potentially thinner slice will be at the top.
Number of Slices
Checking ✓ this option will divide the model into a specific number of slices. The slice thickness will be determined by the Composite Model thickness divided by the Number of Slices defined. This may be a good option to use if the specific slice thickness is not important (for instance if it does not relate to material thickness).
Example
If the Composite Model is 3.96 inches thick and you define 3 Slices then the software will create 3 Component slices each 1.32 inches thick.
Create Boundary Vectors
Checking ✓ this option will cause the slicer to create vector boundaries for each slice. These can be useful for defining the subsequent machining regions required to cut each part. The boundary vectors will be placed on the same layer in the 2D View as the component preview for their associated model slice.
Slice Model
Clicking will apply the choices made in the form and create the Components which represent each slice of the Composite Model.
Note
The Component Tree will retain a copy of the original Components in the part as well as the new Slice Components. This may result in a very thick looking model as all the slices will be added to the original shapes. At this point you can delete, undraw or move Components before proceeding with any additional operations.
Close
Clicking will close the Slice Model form without completing the operation.
Slice Heights
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 many 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.
Controlling Slice Thickness
A specific slice height can be controlled by selecting it from the slice list, updating the value and clicking
Updating the height of a specific slice might potentially adjust the thickness of the surrounding slices
Add New Slices
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
Removing Slices
To remove a slice height select it from the list and press the Delete button. Deleting a slice height will merge the surrounding slices into one slice.
3D View
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.
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.
Trace Bitmap
This tool automatically traces or fits vectors to image files so they can be machined. Use the Import Bitmap tool and select the image in the 2D view, then open Fit Vectors to Bitmap.
After importing an image the Tracing option allows vector boundaries to be created automatically around colored or black and white regions in the image.
Tracing a Selected Area of the Bitmap
You can define an area within the bitmap, such that only that part of the bitmap will be traced. This can be done by selecting the bitmap (if this hasn't been done already), and then clicking and dragging the mouse over the area you want, to define a rectangular region on the bitmap. This will be highlighted with a dashed black rectangle.
Clicking on the Bitmap again will remove a selected area if one has been specified, in which case, the entire bitmap will have vectors fitted to it.
Tracing Black and White Images
When working with Black and White images the slider can be used to change the Threshold and merge the levels of gray between all white (min), and all black (max).
When the image being displayed in the 2D view looks correct then clicking the button automatically creates vector boundaries either around the selected Trace Color or the grayscale.
Tracing Color Images
Color images are automatically reduced to 16 colors and the slider allows the visible number of colors to be set as required. Colors are merged with the closest match.
Colors can be temporarily linked together by clicking the check boxes next to each of the colors displayed. This changes the color displayed in the 2D view to the selected Trace Color. This is very useful for merging similar color's together to allow complete regions to be traced.
If a new Trace Color is selected the linked colors are displayed using this color in the 2D view.
The Reset button unlinks all the checked ✓ colors and the image displayed in the 2D view reverts back to the original 16 color image.
2D View
You can select the colours directly from the image in the 2D View.
Tracing a Selected Area of the Bitmap
You can define an area within the bitmap, such that only that part of the bitmap will be traced. This can be done by selecting the bitmap (if this hasn't been done already), and then clicking and dragging the mouse over the area you want, to define a rectangular region on the bitmap. This will be highlighted with a dashed black rectangle.
Clicking on the Bitmap again will remove a selected area if one has been specified, in which case, the entire bitmap will have vectors fitted to it.
Fitting-Options
The options available on this form control how closely the vectors fit / follow the selected color boundaries and these can be modified to obtain improved results.
Corner Fit
The Corner Fit control determines how accurately the vectors are fitted to the corner edges in an image.
Noise Filter
The Noise Filter slider controls the minimum size of pixels that are traced / vectorized, preventing small unwanted vectors or noise being created.
Bitmap Fading
Preview
This will preview the result of the tracing of the bitmap. If you are not happy with the result provided, you can alter the settings and click on the button again to get an updated result.
Apply
When you are happy with the result of the preview you can click on the button to keep it.
How to Get Started
The first stage in any project is to create a new blank part or import some existing data to work with. At this stage a number of parameters need to be defined relating to the size of the part and its position relative to the datum location on the CNC machine. Later, once the part has been defined and you have started working, you may want to change the size of the material, import additional data and generally manage the project operation. In this section of the manual the initial creation of a part will be covered along with all the icons which appear under the File Operations section of the Drawing Tab.
When you first start the program you will see the Startup Task options on the left hand tab and also a list of your 4 most recently opened VCarve Desktop parts (this is a rolling list that will be populated each time you run the software and may initially be empty).
Startup Tasks and Recently Opened Files
When you first start the program you will see the Startup Task options on the left hand tab and also a list of your most recently opened VCarve Desktop parts.
The first choice is whether you want to Create a new file or Open an existing one. Creating a new file allows you specify a size and location for a blank work area, set your material thickness and also set the model quality and even the shading color/material. The process to do this will be covered in the next section (Job Setup Form Options).
The second choice, Open an Existing File, will allow you to open a pre-created file from your computer. This may be a file you previously created (*.crv3d or *.crv). Alternatively, it might be a 2D vector layout from another CAD system (*.dxf, *.eps, *.ai and *.pdf). A CRV3D or CRV file will have the necessary information for material size etc. already embedded in it. The 2D formats will import the data at the size and position it was created but will require you to go through the Job Setup form to verify/edit all the parameters for the part.
Video Tutorials
The Tutorial Video Browser will open your default web browser (typically Internet Explorer, Chrome or Firefox - depending on your Windows setup and personal preference). The web browser offers a number of tutorial videos and associated files, presented either by project or feature category to help you to learn about the software. You will initially need internet access to watch or download the videos or files, but, once downloaded, the materials can be used offline.
Online Resources
This section includes direct links to useful websites and web resources - including clipart and projects for you to purchase, download and incorporate into your own designs. These links will also open in your default web browser and you will need internet access to use them.
Interactive Vector Trim
The interactive trimming tool allows the user to just click on sections of vectors they want to delete.
The program finds the closest intersections either side of the clicked portion of the vector and removes the piece of the vector between the intersections. Optionally, when the form for this command is closed, the program can rejoin all the remaining trimmed pieces automatically.
Without using this tool, to remove an overlapping section of a vector, the user would need to insert extra nodes into both vectors, manually delete the intermediate sections and then manually join the resulting pieces. These operations can be performed with a single click using this tool.
When the tool is selected the cursor changes into a 'closed' scissor shape. When the cursor is moved over a vector suitable for trimming the scissors 'open' to show you can click and trim.
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.
Note
If you try to trim a group then the group will flash pink. This indicates that it cannot be trimmed unless it first has to be ungrouped
Rejoin Trimmed Sections
Allows the user to select whether the program will automatically try to rejoin trimmed vectors when the form is closed. For most simple cases like that shown above with the overlapping rings, this option can be left checked ✓. If you have an example where for instance many trimmed lines meet at the same point, you may want to uncheck this option and rejoin the vectors manually.
Job Setup - Single Sided
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.
In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a 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.
Job Type
Single Sided job type should be used when design only requires the material to be cut from one side. This is the simplest type of job to design and machine.
Double Sided Job type is useful when it is desired to cut both sides of your material. Aspire allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file.
Rotary job type enables the use of a rotary axis (also called a 4th axis or indexer).Aspire will provide alternative visualisation, simulation and tools appropriate for rotary designs.
Job Size
This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).
It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).
VCarve Desktop only supports job sizes up to a maximum of 25 inches square without tiling.
You can cut jobs larger than this limit but you will need to use the Toolpath Tiling feature to cut the job in sections.
Z-Zero Position
Indicates whether the tip of the tool is set off the surface of the material (as shown in the diagram) or off the bed / table of the machine for Z = 0.0.
XY Datum Position
This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's position.
Use Offset
This option allows the datum position to be set to a value other than X0, Y0.
Design Scaling
When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click
Modeling Resolution
This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.
As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.
The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.
As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.
Appearance
Clicking will pop up a dialog allowing you to set the color or material effect which will be applied to the base 3D model. It is possible to change this at any time and also to apply different colors and materials to different Components using the Component manager. See Preview Toolpaths to learn more about different material settings and adding custom material effects.
Importing External Models in a Rotary Project
Importing Full-3D models
This section will present the process of importing the Full-3D STL model into rotary project, using a table leg as an example.
Overview
There are two basic use cases when importing an external model into the rotary job. The first case involves bringing a model designed for this particular job in another software. Thus the dimensions of the imported piece may already be correct and it can be desired to use them for the size of project. The second use case is when importing a stock model that would have to be scaled to fit on particular machine.
Aspire uses following workflow that covers both of those cases:
- Setting-up rotary project
- Choosing file for import
- Orientating the model in material block
- Scaling the model
- Finishing the import
Setting up a rotary project
Create a new job using the Job Setup form. It is important to set the job type as rotary to ensure a proper import tool is used in the next step.
If the dimensions of the project are already known, they could be specified directly.
If it is desired to fit the model to a given machine or stock available, set both the diameter and length to maximum. During import the model will be scaled to those limits.
If it is desired to use the imported model size, any size can be specified at this time. During the model import the project can be automatically resized to match the model dimensions.
In this example it was desired to fit the model into a specific stock size with a Diameter of 4 inches and a Length of 12 inches. XY origin was set to centre.
Importing the file and orientating it
To start the importing process, use Import a Component or 3D Model tool from the Modelling tab
Make sure that the Imported model type is set to Full 3D model .
The first step is to position the imported model within the material. This step is necessary as this information is not present in the imported file. When the model was opened, the import tool chose the initial orientation, as can be seen below.
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.
Scaling imported model
Once model has been positioned as desired, its size can be taken into account.
By default the tool will assume that imported model is using the same units as the project. If that is not the case, model units can be switched. In this example project was set-up in inches, while imported model was designed in mm. After switching model becomes considerably smaller and a red cylinder, representing current material block is shown, as can be seen below.
At this point it is possible to specify the model size, in terms of diameter and length. This can be done manually by typing desired dimensions, or by fitting to material. If Lock ratio option is selected, the ratio between diameter and length is kept. One can also tick Resize material block option. If it is selected, the material block will be scaled to match current size of the model, after OK is clicked.
If it is desired to use model size as material block size, one can just make sure units are correct, then tick Resize material block option and press OK.
If it is desired for the model to fit material, one could click Scale model to fit material and tick Resize material block.
In this example model was fitted to material. Since in this case length of the piece is limiting factor and lock ratio is maintained, this results in model having considerably smaller diameter than material block. Hence Resize material block option was ticked.
Finishing import
After pressing OK the model will be imported as a component. It is possible to modify it as any other component or add pieces of decorative clipart onto its surface if desired.
It is important to keep in mind the distortion caused by the wrapping process. That means that wrapped toolpaths will match flat toolpaths only at the surface of the blank. The closer to the rotation axis (i.e. deeper) the toolpath is, the more it will be 'compressed'. This fact have a profound implication for 3D toolpaths. Consider the example shown below.
As can be seen if there is substantial difference in diameter in different parts of model, generating one 3D toolpath for whole model will result in wrapped toolpath being overly compressed. Thus it is usually better to create boundaries of regions with significantly different diameter and generate separate toolpaths using correct settings for each diameter.
Importing Flat Models
This section will present a process of importing Flat STL model into rotary project. Flat models are similar to decorative clipart pieces provided with Aspire and are supposed to be placed on the surface of modelled shape.
To start the importing process, use Import a Component or 3D Model tool from the Modelling tab
Make sure that Imported model type is set to Flat model
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
Crash Handling
In the unfortunate event of the software crashing,
- We try to save unsaved changes, so that your data isn't lost.
- Provide an easy way for you to report the crash so that we can work on a fix.
Project Saving
If you're working on a job and the software crashes, the first thing it will try to do is to save your project. The project will be saved alongside your original to avoid accidentally corrupting your original file.
Report the crash
A dialog will pop up asking you to upload the crash information which will help us track down the issue. Any information you can think of would be greatly appreciated and will help us fix the issue in a timely manner.
Description
Please try to remember what you were doing at the time, and describe it for us. Please include any information you can think of. Any bit of information can help us track the issue quicker, so we greatly appreciate that.
Information
You can include your name and e-mail to allow us to get back to you with questions in case we need more information. For example, we may need the project that you were working on. This data will not be used for any purpose other than to help us track down the issue.
Internet
You will need to be connected to the internet for this to work. If not, you can still send the generated zipped report to support@vectric.com. The report can be found in the Application Program Data (Accessible through the menu 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.
Auto Layout Text
This option automatically sizes a block of text to fit inside the boundary box (width and height limits) of a selected vector or vectors. If no vectors are selected the text is scaled to fit the size of the material.
Entering Text
The procedure for Drawing Text in the 2D Window is:
- Select the vector inside which the text is to be fitted
- Click the Draw Text icon
- Enter the required text content
- Select the font either True Type or Single Line as required and alignment options
The button opens a larger text entry window that makes it easier to enter text that needs to run on longer line lengths.
Font Selection
Vertical Fonts
Fonts that start with the @ character are drawn vertically downwards and are always left justified
Engraving Fonts
The Single Line Radio Button changes the Fonts list to show a selection of fonts that are very quick to engrave.
This example shows text (in an Engraving Font) drawn in an ellipse. The bounding box of the ellipse is used for the layout:
Text Alignment
Positions text relative to the selected bounding box or material size with options for left, center and right aligned.
Bounding Box Dimensions
These are the actual size of the box into which the text will be fitted. If the text is scaled interactively (by left clicking twice on the text) or precisely using the scale tool, the new bounding box is updated and displayed as a light gray rectangle.
Margin Size
The distance between the text and the bounding box where:
- None - Scales text to fit the rectangle width or height of the bounding box
- Normal - Scales text to fit within 80% of the bounding leaving a 10% border to the left and right.
- Wide - Reduces the size to 60% of the rectangle width leaving a 20% border to the left and right.
Vertical Stretch
When the text fits the width of the box and there is space above and below it, the text can be made to fill that vertical space using one these methods:
Horizontal Stretch
When the text fits the height of the box and there is space at the sides, the text can be made to fill that horizontal space using one these methods:
Edit Text
To edit text properties or content of previously created text:
If the Create Text form is open, click the text you wish to edit or
If the Create Text form is closed, click the left mouse button on the text in the 2D View to select it before opening this form. The form will now allow you to edit the properties of the selected text.
Spell Checker
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
Edit Picture
The Edit Picture form allows you to add a border to, and edit the properties of a selected bitmap.
Contrast
This slider adjusts the contrast. A higher contrast emphasises the differences between the light and dark parts of the image.
Brightness
This slider adjusts the brightness of the image.
Gamma
This slider adjusts the gamma correction applied to the image. This can make an image look lighter or darker whilst maintaining detail.
Invert
Inverts the colors in the image. White becomes black and black becomes white
Grayscale
Makes the image black and white.
Add Border
Fades the edges of the image based on the border type and the width of the fading.
Edit Sheet - Rotary
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.
In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.
Job Size
Length
Length of the material
Diameter
Diameter of the material
Units
Whether the job units are measured in mm or inches
Z Zero Position
Indicates whether the tip of the tool is set off the rotation axis (as shown in the diagram) or off the surface of material for Z = 0.0. For the best accuracy using Cylinder Axis option is recommended
XY Datum Position
This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's position.
Use Offset
This option allows the datum position to be set to a value other than X0, Y0.
Orientation
This option selects along which axis the material block will rotate.
- Selecting Along X Axis means that X coordinates represent movement along the cylinder, whereas Y coordinates represent the angle around the cylinder.
- Selecting Along Y Axis means that Y coordinates represent movement along the cylinder, whereas X coordinates represent the angle around the cylinder.
Flip Design
When this option is enabled, the design will be flipped when the orientation is changed
Design Scaling
When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click
Modeling Resolution
This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.
As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.
The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.
As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.
Appearance
Clicking will pop up a dialog allowing you to set the color or material effect which will be applied to the base 3D model. It is possible to change this at any time and also to apply different colors and materials to different Components using the Component manager. See Preview Toolpaths to learn more about different material settings and adding custom material effects.
Draw Star
Stars can be created interactively with the cursor and Quick Keys, or by entering the number of points, exact coordinates and outer radius and inner radius percentage using typed input.
Interactive Creation
The quickest and easiest way to create a star is by clicking and dragging the shape to size in the 2D View using the mouse.
- Click and hold the left mouse button to indicate the center point.
- Drag the mouse while holding down the left mouse to required radius.
- Release the left mouse button to complete the shape.
Note
Holding Alt and dragging creates a star from the middle point.
As the cursor is dragged across the screen so the outer radius is dynamically updated. The increments will depend upon your snap radius and the job size.
Quick Keys
Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.
- Left-click and drag out your shape in the 2D View.
- With the left mouse button still pressed, enter a quick key sequence detailed below.
- Release the left mouse button.
Default
By default, entering a single value will be used to set the outer radius of your star. While you are dragging out the star, type Radius Value Enter to create a star with the precisely specified outer radius.
Example
- 2 . 5 Enter - Creates a start with an outer radius of 2.5 all other settings as per the form
Specifying Further Properties
By using specific letter keys after your value, you can also indicate precisely which property it relates to.
Note
When specifying multiple properties with quick keys, it is still important that they are entered in the order indicated in the table below.
- Value D - Creates a start with the outer Diameter (D) specified with all other properties as per the form
- Value I Value R - Creates a star with the inner radius percentage (I) and the outer radius (R). The inner radius is defined in terms of a percentage of the outer radius or diameter. All other properties are as per the form.
- Value P Value R - Creates a star with the specified number of points (P) and the outer radius (R).
- Value P Value I - Creates a star with the specified number of points (P), inner radius percentage (I) and the outer radius (R).
Examples
- 1 R - Outer radius 1, other properties as per form
- 1 D - Outer diameter 1, other properties as per form
- 6 P 1 R - A 6 pointed star with an outer radius of 1
- 6 P 2 5 I 4 D - A 6 pointer (P) star with an outer diameter (D) of 4 and an inner diameter that is 25% of the outer (i.e. 1).
Exact Size
Stars can also be drawn by entering the Number of Points, Center Point, Outer Radius and Inner Radius Percentage.
- Click to update the star.
Help
Help Contents | Displays an online version of the full reference manual that documents every feature and option available in the software. Note The reference manual is not intended as a User Guide or introductory training resource - please don't forget about the Getting Started guides and the extensive video tutorial library on your install media. |
Keyboard Shorcuts | Displays the Shortcut Keys |
Video Tutorial Browser... | Access the tutorials |
What's New | See a summary of the new features added in major and minor updates. |
Release Notes | See the list of issues fixed and enhancements in patch updates. |
Third Party Licences | Display a list of all the third party software used to help create VCarve Desktop. |
Enter License Code | Displays the License Dialog used for entering license or module details. |
View the Vectric Online FAQ... | Displays the Frequently Asked Questions (FAQs) |
View the Vectric User Forum... | Opens the Vectric User Forum in your Web Browser if you have an Internet Connection. Everyone should join the Forum to engage with other users and benefit from each others tricks and tips! |
Visit Vectric Support online... | Opens the Vectric Support Website in your Web Browser if you have an Internet Connection. |
Visit Vectric User Portal... | Opens the Vectric User Portal in your Web Browser if you have an Internet Connection. Download software installation files, activation codes and Clip Art included with the software. |
Post Processor Editing Guide | Opens the page explaining how to create and edit your own post processors. |
Migrate From Older Version | Opens a dialog to enable the settings in the last version of VCarve Desktop to be copied to the latest version. |
Check for Updates | Try this periodically to check (through the Internet) if an update is available for your software. |
Run Kickstarter | Opens a wizard allowing the user to get started. |
About VCarve Desktop... | This window displays the version of the software being used, to whom the software is license and the type of license. |
Post-Processor Content
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.
Machine Configuration Post-Processor
In the Machine Configuration Management dialog, you have the ability to define a fixed version of the post-processor for use. Viewing this post-processor through there will be showing you the content of that version you have selected, and not the contents of the latest version. If you want to see the contents of the latest version, then you need to View the post-processor through the Post-Processor Management dialog.
POST_NAME
If you would like to copy the contents of this post-processor and use it, you will need to add a POST_NAME statement at the top of the file. This will be done automatically for you if you choose the 'Customise' option instead.
You can cut and paste content in text form to the clipboard of your computer.
Custom Post-Processor
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.
License Dialog
The License Dialog is used to set the details you need to activate the software. This dialog can also be used to activate optional modules. The page that initially appears will give you the option to set your license details either automatically from your V&Co account or manually.
The "Online Method" section below covers the process to follow if Online is selected.
The "Manual Method" section below shows the process to follow if you wish to type in your license details manually or do not have an Internet connection available.
Online Method
This method will allow you to retrieve your details automatically from your V&Co account. To use this select 'Online' and then click on the form. The online section of the form will then be displayed.
Pressing 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 Desktop 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 Desktop to retrieve your license details automatically.
At this point VCarve Desktopshould 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 can be pressed to activate these and proceed to the summary page.
Note
If there is only a single license available on your account the above page is skipped and the summary page (below) will already be displayed.
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 VCarve Desktop 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 Desktop is restarted.
Manual Method
The manual method allows entry of license details without requiring an Internet connection.
There are 2 methods for entering a licences,
- Loading from a File
- Typing or Copying the values into the text fields
Load from File
You can choose to download a vlicence file from your V&Co account.
There are 2 ways to use this file
- Double-click the file to open it with the software
- Go through the License Dialog wizard and click to Load the vlicence file.
Multiple Software Installations
If you have a previous version of the software installed, please make sure you use the correct installation of the software to open the vlicence file with.
Manual
License Data
You can get the License Data from your V&Co account and enter it using the Enter License Data option.
Example License Data
---BEGIN VECTRIC LICENCE--- eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ0123456789eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ012345 6789eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ0123456789eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ01 23456789eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ0123456789eyJ2ABCDEFGHIJKLMNOPQRSTUVWX YZ0123456789eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ0123456789eyJ2ABCDEFGHIJKLMNOPQRST UVWXYZ0123456789eyJ2ABCDEFGHIJKLMNOPQRSTUVWXYZ0123456789== ---END VECTRIC LICENCE---
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.
Example Registered User Name & License Code
Registered User Name My Machine Test - 00100 License Code ABCDEF-GHIJKL-MNOPQR-STUVWX-YZ0123-456789-ABCDEF-GHIJKL-MNOPQR-STUVWX
Copying the License Code
You can copy the entire code into the first field and will automatically fill the rest of the text fields.
If the product is already licensed then a module code can be entered at this stage instead of the product code. If you wish to manually activate both a product and module code the product code should be added here and there will be an opportunity to add the module code later.
Pressing will set the license and display the summary screen.
Adding Module
The summary screen shows the current licensed user and has an button to allow additional modules to be added. Pressing this button will display the manual entry form again and allow the module details to be entered.
If the licensed user is changed or a new module is added a restart will be required for these to take full effect. In this case a check box will appear allowing you to restart automatically. If this is checked then when you press the finish button the program will automatically be restarted to apply the license changes. If you do not select this option the license changes take effect the next time the program is restarted.
Edit Sheet - Double Sided
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.
In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.
Job Type
Single Sided job type should be used when design only requires the material to be cut from one side. This is the simplest type of job to design and machine.
Double Sided Job type is useful when it is desired to cut both sides of your material. Aspire allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file.
Rotary job type enables the use of a rotary axis (also called a 4th axis or indexer).Aspire will provide alternative visualisation, simulation and tools appropriate for rotary designs.
Job Size
This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).
It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).
VCarve Desktop only supports job sizes up to a maximum of 25 inches square without tiling.
You can cut jobs larger than this limit but you will need to use the Toolpath Tiling feature to cut the job in sections.
Z Zero Position
Indicates whether the tip of the tool is set off the surface of the material (as shown in the diagram) or off the bed / table of the machine for Z = 0.0.
Zero off same side
This option allows Z Zero to reference the same physical location, regardless whether material is flipped or not
XY Datum Position
This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's position.
Use Offset
This option allows the datum position to be set to a value other than X0, Y0.
Flip Direction Between Sides
This section gives choice between horizontal and vertical flipping when changing machining side. Aspire uses that information to correctly manage the alignment of the geometry relating to each side.
Design Scaling
When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click
Modeling Resolution
This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.
As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.
The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.
As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.
Appearance
Clicking will pop up a dialog allowing you to set the color or material effect which will be applied to the base 3D model. It is possible to change this at any time and also to apply different colors and materials to different Components using the Component manager. See Preview Toolpaths to learn more about different material settings and adding custom material effects.
Save Toolpaths
This option allows toolpaths to be saved in the appropriate file format needed to drive the CNC machine. Toolpaths can be saved as individual files for each tool used or as a single file containing multiple toolpaths for CNC machines that have automatic tool changers.
Save Option
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 button.
Postprocessor selection and association
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.
Selected Toolpath
Saves only the selected toolpath
Visible Toolpaths To One File
Saves all of the visible toolpaths to a single file. Requires that the selected toolpaths uses the same tool, or the use of an automatic tool changer (see below).
Visible Toolpaths To Multiple Files
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.
Automatic Tool Changing Support
CNC Machines that have Automatic Tool Changing (ATC) capabilities can work with a single file that contains multiple toolpaths, each having a different tool number.
The postprocessor must be configured to support ATC commands for your CNC machine. Contact your software or machine supplier for more details.
- The procedure for saving these toolpaths is,
- Use the Up and Down arrows to order the toolpath list in the cutting sequence required.
- Tick each toolpath to ensure it is drawn / visible in the 3D window as shown:
- Click on the Save option and the Save Toolpaths form is displayed. Select the option Output all visible toolpaths to one file
The names of the toolpaths that will be written into the file are displayed along with the tool number in square brackets [1]. If a calculated toolpath is not required, simply tick to undraw it.
Click the button Enter a suitable Name and click the button
Error Messages
The postprocessor automatically checks to ensure:
- It has been configured for saving files that include ATC commands
- A different tool number has been defined for each different cutter being used.
An error message will be displayed to indicate the problem if either of these items is not correct.
Create Text
This form allows text to be created at any height using the units the model is being designed in.
Entering Text
To enter text:
- Click in the 2D view to choose the anchor position
- Enter the text in the Text box
- Edit the styling options. All changes are automatically applied
Font Selection
Vertical Fonts
Fonts that start with the @ character are drawn vertically downwards and are always left justified.
Engraving Fonts
The Single Line Radio Button changes the Fonts list to show a selection of fonts that are very quick to engrave.
Text Alignment
Positions text relative to the full body of text, this only has a noticeable effect when writing multiple lines of text.
Anchor
Sets the position of your text block. Either enter values directly, or use the mouse cursor to set the position values interactively:
- For new text simply left click in 2D view in the desired location
- For existing text object, left click the anchor point handle and drag it to the desired location
Editing Text
To edit text properties or content of previously created text:
- If the Create Text form is open, click the text you wish to edit or
- If the Create Text form is closed, click the left mouse button on the text in the 2D View to select it before opening this form. The form will now allow you to edit the properties of the selected text.
Spell Checker
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
2D Profile Toolpath
Profile Machining is used to cut around or along a vector. Options provide the flexibility for cutting shapes out with optional Tabs / bridges plus an Allowance over/undercut to ensure perfect edge quality.
Profile toolpaths can be outside, inside or on the selected vectors, automatically compensating for the tool diameter and angle for the chosen cut depth.
When working with open vectors the profile toolpaths can be to the Left, to the Right or On the selected vectors.
Clicking this icon opens the 2D Profile Toolpath form which is shown at the right; the functions in this form are described on the following pages.
If you have vectors which are nested (like the letter 'O'), the program will automatically determine the nesting and cut the correct side of the inner and outer vectors. In addition, the program will always cut the inner vectors before the outer vectors to ensure the part remains attached to the original material as long as possible.
Cutting Depths
Start Depth (D)
This specifies the depth at which the toolpath is calculated from.
When cutting directly into the surface of a job the Start Depth will often be 0. If machining into the bottom of an existing pocket or 3D region, the depth needs be entered.
Cut Depth (C)
The depth of the toolpath relative to the Start Depth.
Pass Depth Control
When a toolpath is created, the Pass Depth value associated with the selected tool (part of the tool's description) is used to determine the number of passes needed to profile down to the specified Cut Depth. However, by default the software will also modify the precise step down by up to 15% in either direction, if by doing so it is able to total number of passes required to reach the desired cut depth. It is nearly always desirable to benefit from the significantly reduced machining time of cutting using less passes if possible. Nevertheless, there are some occasions where the exact step down for a given profile pass needs to be more precisely controlled - when cutting into laminated material, for example. The Passes section page indicates how many passes will be created with the current settings.Thebutton will open a new dialog that enables the specific number and height of passes to be set directly.
Specify Pass Depths
The Pass Depths section at the top of the form shows a list of the current pass depths. The relative spacing of the passes is indicated in the diagram next to the list. Left click on a depth value in the list, or a depth line on the diagram, to select it. The currently selected pass is highlighted in red on the diagram.
To edit the depth of the selected pass, change the value in the Depth edit box and click .
The button will delete the selected pass.
The Passes button will delete all the passes.
To add a new pass, double left click at the approximate location in the passes diagram that you wish to add the pass. A new pass will be added and automatically selected. Edit the precise Depth value if required and then click .
The Set Last Pass Thickness option will enable an edit box where you can specify the last pass in terms of the remaining thickness of material you wish to cut with the last pass (instead of in terms of its depth). This is often a more intuitive way to specify this value.
Pass Depth List Utilities
Note
Setting the number of passes with either of these utilities will discard any custom passes you may have added.
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.
Machine Vectors...
There are 3 options to choose from to determine how the tool is positioned relative to the selected vectors.
Outside
Inside
On
Direction
Can be set to either Conventional or Climb machining where the cutting direction depends upon the strategy selected - see above for details. Using Climb or Conventional cutting will largely be dictated by the material is being machined and the tooling.
Allowance offset
An Allowance can be specified to either Overcut (negative number will cut smaller) or Undercut (positive numbers will cut larger) the selected shape. If the Allowance = 0 then the toolpaths will machine to the exact size.
Do Separate Last Pass
A separate allowance can be specified for the last pass. If this allowance is given then all but the last pass will be undercut by the specified allowance with the final pass being the only pass which cuts to size.
Note
This is intended to be just a thin skin of material to be cut away as the tool will have to cut through this allowance at the full depth of the cut where all the previous passes undercut. There will be a warning displayed if the last pass allowance is greater than 1/3rd of the tool diameter but the last pass allowance should ideally be kept a lot smaller than this. Keeping this as small as possible reduces the chances the final pass will fit in areas where the previous passes will not and reduces the amount of material the last pass is having to cut through. If using a last pass allowance for the toolpath you should check that you are happy with the amount of material left for the last pass to cut through. The toolpath will fail to calculate if the last pass is cutting a significant distance into material which has not been cleared by the previous passes.
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 Vector Start Point
Use Start Point can be selected to force the toolpath to plunge and start cutting at the first point on the shape. This is very useful if you need to ensure the cutter doesn't plunge onto a critical part of the job. For example, setting the Start Point to be on a corner will often be the best position to plunge and cut from as this will not leave a witness / dwell mark on the machined surface.
The Start Points are displayed as Green boxes on all vectors when this option is selected. Start Point on a vector can be moved using the Node Editing Tools. Select Node Editing cursor or press N. Place the cursor over the node to be used as the Start Point. Click Right mouse button and select Make Start Point (or press P) Remember, you can also insert a new point anywhere on a vector using the Right mouse menu or pressing the letter P - this will insert a new point and make it the start point.
Note
Selecting Use Start Point may result in less efficient toolpaths (increased cutting times) because it may take the machine longer to move between each shape being cut. If this option is not selected the software will try to calculate the shortest toolpath, minimizing the distance between link up moves. But the downside is that the cutter may plunge/mark important surfaces on the machined edge.
Tabs (Bridges)
Tabs are added to open and closed vector shapes to hold parts in place when cutting them out of material.
Add tabs to toolpath
Checking ✓ the Add tabs option will activate tab creation for this toolpath. The Length and Thickness specify the size of each tab. Checking ✓ the Create 3D Tabs option will create 3D Tabs, the difference between this and 2D Tabs is described below.
Create 3D Tabs
When this option is selected the tab will be triangular in section. This is shape is created as the cutter ramps up to the specified Tab Thickness then down the other side. The 3D Tabs will often allow the machine to run quicker and smoother because it does not have to stop to move in Z at the start and end of each tab.
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.
Profile Options
The Profiling options section of the toolpath form contains five additional pages, each of which allows a particular set of Profile machining options to be specified. The precise number of option pages will depend on which Toolpath strategy you are currently using. The full range of option pages are:
- Ramps
- Leads
- Order
- Start At
- Corners
These help control ways to ensure the parts are held in place and machined as easily as possible while ensuring the highest quality edge finish.
Each set of options can be accessed by the tabs at the top of the Profile options section.
Ramp
Ramp moves are used to prevent the cutter from plunging vertically into the material. The cutter gradually cuts at an angle dropping into the material significantly reducing cutter wear, heat build-up and also the load on the router spindle and Z axis of the machine. If multiple passes are required due to the Pass Depth being less than the Cut Depth, the ramp moves are applied at the start of each level. All ramp moves are performed at the plunge rate selected for the current tool.
Smooth
This option creates a smooth ramp into the material using either the specified Distance or Angle.
When a Lead In distance has been specified, the option Ramp on Lead In disables the distance and angle options and automatically limits the ramp moves to only be on the lead in portion of the toolpath.
Zig Zag
This option ramps into the material by Zig-Zag backwards and forwards using either the specified Distance or Angle and Distance.
The Distance option ramps into the material, zigging for the specified distance in one direction then zagging back over the same distance.
The Angle option is typically used for cutters that cannot plunge vertically but have an entry angle specified by the manufacturer.
Spiral
Checking ✓ this creates a continual spiral ramp, these are only available when the toolpath does not include lead in moves.
This option ramps into the material over the complete circumference of the profile pass. The angle is automatically calculated to ramp from the start point to full depth over the perimeter distance around the job.
The rate at which the cutter ramps into the material is determined by the Pass Depth specified for the cutter. For example, Spiral Profiling 0.5 inch deep with a cutter that has a Pass depth of 0.5 or greater will spiral down in 1 pass. Editing the Pass depth to be 0.25 inch results in the 2 spiral passes around the profile.
Leads
Lead in / out moves can be added to profile toolpaths to help preventing marking the edges of components with dwell marks that are typically created when a cutter is plunged vertically on the edge of the job.
Straight Line Lead
This option creates a linear lead onto the cutter path using the Angle and Lead length distance specified.
The toolpath will lead onto the selected edge at the specified Angle.
Checking ✓ the Do lead out option results in an exit lead being added at the end of the toolpath off the machined edge.
The Overcut Distance forces the cutter to machine past the start point and is often used to help produce a better edge quality on parts.
Circular Lead
This option creates an arc lead onto the toolpath using the Radius and Lead length distance specified.
The 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.
Order
The order tab allows you to specify the approaches the program will use to determine the best order to cut your vectors. You can specify multiple options, in which case the program will calculate the result of using each option and select the one which results in the shortest machining time.
Vector Selection Order
This option will machine the vectors in the order in which you selected them. If you have vectors inside each other (like in the letter 'O'), the inner vector will always be machined before the outer one regardless of the selection order.
Left to Right
This option will join up parts on the left of the material first and move across to the right.
Bottom to Top
This option will join up parts on the bottom of the material first and move up to the top.
Grid
This option will join using a grid based approach with the size of the grid based on the size of the parts. The algorithm will try to join up parts within a particular section of the grid before moving on.
Start At
Keep Current Start Points
The start point of the vector will dictate the start of the toolpath.
Optimize Start Points
The software will automatically attempt to optimize each profile start position based on speed of completing the job.
Closest on Bounding Box
Influence the start point by defining which part of the bounding box of the profiled vector it should start near.
This will look for the nearest point, from all of the spans' endpoints, and will start the toolpath from that point.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Project toolpath onto 3D Model
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.
Note:
When a toolpath is projected onto the 3D model, its depth is limited so that it does not exceed the bottom of the material.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Chamfer Toolpath
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.
Cutting Depths
The Start Depth (D) specifies the depth at which the top of the chamfer should start.
Vector Selection
To create the toolpath you must first draw and then select the vectors you wish to create the chamfer on.
Tool
Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.
Chamfer Dimensions
The chamfer dimensions control the shape of the created chamfer.
Angle (A)
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.
Width (W)
The width determines the horizontal size of the chamfer. If the angle is set then changing the width will change the cut depth proportionally.
Cut Depth (C)
The Cut depth is the height of the chamfer. If angle is set then changing the cut depth will change the width proportionally.
Max Cut Depth
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.
Overcut
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.
Note
The length of the side of the tool is unknown and so when specifying an overcut distance you should always ensure that the cutting edge of the tool is long enough to accomodate the overcut distance.
Chamfer Type
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.
Both options can be used together to generate different chamfer styles.
Cut Direction
The cut direction may be set to either climb or conventional milling.
2D Preview
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.
Use Vector Selection Order
If this option is checked, ✓ the vectors will be machined in the order you selected them. If the option is not checked the program will optimize the order to reduce machining time.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Estimating Machining Times
This option estimates the machining times for all calculated toolpaths based on the feed rates specified for each tool. The estimates for individual toolpaths plus the overall machining time of all visible toolpaths are calculated using the user defined Rapid Rate moves and Scale Factor.
Times
The estimated machining times are displayed in Hours: Minutes: Seconds
Rapid Rate
The maximum feed rate at which the machine runs for rapid moves, typically specified using a G0 or G00 move
Scale Factor
The nature of different styles of toolpaths means that they may be simple 2D cuts or require simultaneous 3-axis moves, the more complex the toolpath then the more chance the CNC machine may not actually achieve the programmed feed rates. This can be compensated for by multiplying the times by the Scale Factor.
The scale factor in the program lets you approximate this slowdown for your machine, but it will vary depending on the type of work you are doing. Many people will use one scale factor for simple 2d work and another for 3d or VCarving. The best way to calculate it is just to take a note of estimated and actual machining times of a period of time.
For machines where the controller provides an estimated machining time, these should be more accurate as the controller can determine where the machine is accelerating / decelerating and take account of this.
2D View Controls
See also the Rulers, Guides and Snap Grid section.
Pan | Click and hold the Left mouse button and drag the mouse about to Pan - Esc to cancel mode Shortcut: Click and drag the Middle mouse button or if using a 2 button mouse, Hold Ctrl + drag with Right Mouse button. | ||
Zoom Interactive | Mouse with Middle Wheel - Scroll wheel in / out Mouse without Middle Wheel - Hold Shift + Push / Pull with Right Mouse button. | ||
Zoom Box | Click top left corner, hold mouse down and drag to bottom right corner and release. Clicking the left mouse button will zoom in, Shift + click will zoom out. | ||
Zoom Extents | Zooms to show material limits in the 2D window | ||
Zoom Selected | With objects selected Zooms to the bounding box of the selection |
Sheets
When there are multiple sheets in the job then the outline of the sheets is shown in the 2D view.
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 or by double clicking on the sheet in the 2D view.
Undo Operation
Clicking this option steps backwards through the design changes made by the user.
Draw Arc
The Create Arc tool allows a single arc span to be created using precise values, or dynamically within the 2D View.
Through 3 Points
- Left click the mouse in the 2D View to set the start point of an arc.
- Click again to set the end point position.
- Move the mouse and click a third point to set the arc's radius.
Center, Start and End
- Left click the mouse in the 2D View to set the center point of the arc.
- Click again to set the start point of the arc.
- Move the mouse and click a third point to set the end point of the arc.
Note
Clicking the Right mouse button or pressing the Esc key will complete the arc drawing if possible and close the form.
Exact Size
Precise values for the start and end point positions (in absolute X Y coordinates) and either the radius or the height of the arc can be entered in the form directly. Click to draw and arc using these values.
Material Setup
The Material Setup section of the Toolpaths tab provides a summary of the current material settings. Some of these values will have been initially set when the job was first created (see Job Setup for more information). When you come to creating toolpaths, it is important to review this information and ensure it is still valid and also to set the machining clearances. To access all these properties for editing, click on the button to open the Material Setup form:
Different form is displayed depending on the job type:
Toolpath Tiling Manager
Using the Toolpath Tiling options it is possible to machine objects and designs that are many times larger than the available area of your CNC machine bed. This process is also invaluable if the maximum size of your material pieces are limited. In both cases, a much larger project can still be achieved by breaking the toolpath down into manageable tiles or strips, each of which can fit within the machinable area of your CNC machine, or on the available material blocks. Once cut, the tiles can then be re-assembled to form the finished piece.
The process of tiling begins by creating toolpaths based on the final object entirely as normal - at this stage you do not need to take any account of the available machining bed size. Once you have calculated required toolpaths, click on the toolpath tiling button in the toolpaths pane to open up the toolpath tiling form.
Tiling Options
There are three layout strategies for tiled toolpaths, the most appropriate one will depend on your machines capabilities and the available material.
Individual Tiles
The first tiling option is for individual tiles. This splits the current job in both X and Y, to form a series of entirely separate toolpaths. This is generally the preferred option if you have independent pieces of material to machine, or if you have a moving-bed type CNC machine that will not allow you to 'overhang' material outside of the machinable area.
With this option selected, you are asked to specify the width and height of each tile, and the required overlap (which will be applied in each direction). Tiles are created from the bottom left of your model. The overlap for independent tiles is particularly important for 2.5D toolpaths that utilize the shape of your tool bit (such as V-bit carving). 2.5D toolpaths will need to 'overrun' the edges of your tile in order to complete their cuts using the side of the bit. For this reason, the overlap distance for Independent Tiles will typically need to be at least equal to the radius of your tool bit.
Feed-through in X or Feed-through in Y
Instead of cutting a series of individual pieces of material and assembling them later, it can also be convenient to cut a single strip of material using a series of set-ups - moving the material through the machinable area between cuts. Aspirespecifically supports this technique using the Feed-through in X/Y options. In these cases you will only need to define either the Tile Width or Height (which corresponds to your intended feed-through distance), as the other dimension is assumed to correspond to the shorter side length of your material and will match the equivalent current job dimension. Similarly, the overlap distance is only applied in the direction of the draw-through. Because you will typically be cutting the same piece of material with each toolpath tile, the overlap distance for Feed-through is not as critical as for Individual tiles and is typically used to allow for a margin of error in your set-up accuracy.
Once you have set your tiling option, click the Update Tiles button to see your settings reflected in the Tile Previews in either the 2D or 3D Views.
Machine smallest tile first
If this option is unchecked then the tiling space is divided into parts of the specified size. Any remainder space is placed at the end. If the option is checked then the remaining space is placed at the beginning.
Tile Previews
The 2D View indicates how the model area is split into tiles. The yellow lines indicate the tile sizes, but the light red areas also indicate the overlap region for each tile.
Double-clicking on a tile will make that tile the active tile.
In the 3D view the toolpaths will be showed tiled, with only the moves that are within the active tile shown.
Simulating Tiled toolpaths
You can also view and simulate individual toolpath tiles in the 3D View. To view the toolpath tiles, simply ensure that the toolpaths are visible (checked ✓ in the Toolpath List) and then select the tile you wish to see either from the Tile Toolpaths form, or the 2D View (see above).
Since tiles are created so that they will all be cut within the same machinable area (i.e. they are all located in a similar position relative to the machining origin), this can make them difficult to visualize using Preview Toolpaths. Simulating each toolpath tile in its absolute position will result in the toolpaths being cut in the same region of your preview block and they will overcut the same area. The Tile Toolpaths form has an option Draw toolpaths in original position for visualization to allow you to simulate the tiles as if they were arranged in their final pattern. With this option enabled, you can visualize how your final piece will look by previewing all your toolpath tiles together, but you should note that it will not reflect the true offset of each toolpath from your machining origin.
Saving toolpath tiles
Provided you have created toolpath tiles using the Tile Toolpaths form, an additional option, Output Tiled Toolpaths, will be available in the toolpath saving form.
It will be checked ✓ or unchecked to match the current state of the Tile Toolpaths check box in the Tile Toolpaths form.
2D Design and Management
The 2D View is used to design and manage the layout of your finished part. Different entities are used to allow the user to control items that are either strictly 2D or are 2D representations of objects in the 3D View. A list of these 2D View entities are described briefly below and more fully in later sections of this manual.
Ultimately the point of all these different types of objects is to allow you to create the toolpaths you need to cut the part you want on your CNC. This may mean that they help you to create the basis for the 3D model or that they are more directly related to the toolpath such as describing its boundary shape. The different applications and uses for these 2D items mean that organization of them is very important. For this reason VCarve Desktop has a Layer function for managing 2D data. The Layers are a way of associating different 2D entities together to allow the user to manage them more effectively. Layers will be described in detail later in the relevant section of this manual. If you are working with a 2 Sided project you can switch between the 'Top' and 'Bottom' sides in the same session, enabling you to create and edit data on each side, and using the 'Multi Sided View' option you can view the vectors on the opposite side. 2 Sided Setup will be described in detail later in the relevant section of this manual.
Vectors
Vectors are lines, arcs and curves which can be as simple as a straight line or can make up complex 2D designs. They have many uses in VCarve Desktop, such as describing a shape for a toolpath to follow or creating designs. VCarve Desktop contains a number of vector creation and editing tools which are covered in this manual.
As well as creating vectors within the software many users will also import vectors from other design software such as Corel Draw or AutoCAD. VCarve Desktop supports the following vector formats for import: *.dxf, *.eps, *.ai, *.pdf, *skp and *svg. Once imported, the data can be edited and combined using the Vector Editing tools within the software.
Bitmaps
Although bitmap is a standard computer term for a pixel based image (such as a photo) in *.bmp, *.jpg, *.gif, *.tif, *.png and *.jpeg. These file types are images made up of tiny squares (pixels) which represent a scanned picture, digital photo or perhaps an image taken from the internet.
To make 3D models simple to Work with, VCarve Desktop uses a method which lets the user break the design down into manageable pieces called Components. In the 2D View a Component is shown as a Grayscale shape, this can be selected and edited to move its position, change its size etc. Working with the Grayscale's will be covered in detail later in this manual. As with bitmaps, many of the vector editing tools will also work on a selected Component Grayscale.
Interactive Selection Mode
The Interactive Move, Rotate, Scale Selection tools can be used to quickly and easily modify vectors and components.
Clicking twice on one of the selected objects and the interactive scaling, movement and rotation handles are displayed in the same way as selecting this icon. Lines, Arcs and Bezier spans will be displayed as dotted magenta lines and text and grouped objects will be displayed as solid magenta lines:
When in this mode the mouse is used to click on one of the handles which has appeared on the selected Vector/s. Each handle is used for a specific editing operation as detailed here:
- Middle - Move the vectors (Hold +Alt Move the selected objects in one axis)
- 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)
To deselect objects,
- Click the white background unless Shift is pressed.
- Press Esc
- Right click menu ► Unselect All
Tool Database - Custom Naming Variables
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.
Creating Custom Variables
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.
Applying Custom Variables
- Click the ‘Edit’ button next to the tool name above the notes field.
- Place cursor where you would like to place value within string
- Right click > Custom Attributes variables > Search and select correct name in list.
Note
Custom variables should be created and then selected from the list rather than entered manually with prefix. This is to prevent conflict with the software’s own pre-set variables. The purpose of custom variables is purely organisational, they cannot action an effect on tool parameters or toolpath output.
- Click ‘Ok’ at the bottom of the form to apply changes.
Import Vectors
This opens the File Open dialog window and allows 2D DXF, EPS and AI and PDF files to be imported into the 2D View. The imported vectors will always be read in at the size and scale they were created in their original design software. Once open they can be scaled and edited in the same way as vectors created in Aspire. All the Vector tools will be dealt with in that section of this manual.
To import toolpaths from PhotoVCarve and Cut3D (.PVC and .V3D file extensions), use File ► Import... ► Import PhotoVCarve or Cut3D Toolpaths from the file menu bar. Any Toolpath data saved as .PVC or .V3D files can be imported and will be visible in the Toolpath List.
See the 3D Toolpath Files section for detailed instructions on importing PhotoVCarve(*.pvc), Cut3D(*.v3d) or Vectric 3D Machinist(*.v3m) files.
Simple Rotary Modelling using 2D Toolpaths
Creating vectors for a basic column
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.
Creating rotary toolpaths
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.
Simulating and saving toolpaths
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.
Contrary to single - and double - sided simulation, rotary simulation is not 100% accurate. For example round holes will appear in rotary view as oval ones, but obviously will be round when part is actually machined.
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.
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.
Note
Tools and values presented in this example are for illustrative purposes only. Size of tools, feed rate, tabs diameter etc. have to be adapted to the material and machine used to ensure safe and accurate machining.
Spiral toolpaths
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.
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.
Getting Started: Online Machine Configuration
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.
Can't find your machine?
If you can't find your machine, you can configure it manually in the next step, or later on through the Machine Configuration Management dialog.
Snapping Options Dialog
To help with drawing, construction and layout, the 2D View has Rulers which are displayed along the top and down the left side of the window. In addition to the Rulers there is the option to use Guidelines and The Smart Cursor to help with construction of vectors or positioning of other objects in the 2D View.
Rulers
The Rulers are permanently displayed in the 2D view to help with positioning, sizing and alignment. The graduated scale automatically uses the units set for the project and zooming in / out shows the sizes in 10ths.
Guidelines
Guide Lines are used to help layout designs and make it very easy to sketch shapes by clicking on the intersections of Guides. Guide Lines are easily be added to the 2D view by pressing the left mouse button down on the appropriate ruler (left if you want a vertical guide and top if you want a horizontal guide) then holding the button down and dragging the mouse into the 2D view.
While dragging a Guide into position it automatically Snaps to the units displayed on the ruler. This snapping behavior can be overridden by holding down a Shift key while dragging the guide. After positioning a Guide it can easily be moved to a new position by clicking the right mouse button on the guide to open the Guide Properties form as shown later in this section. If you hover the mouse over a Guideline then its current position is displayed next to the cursor
Additional guide lines can be added relative to an existing guide line by interactively placing the cursor over an existing guide (the cursor changes to 2 horizontal arrows), Holding a Ctrl key and dragging to the required position. The incremental distance between the guide lines is displayed next to the cursor. Releasing a Ctrl key changes to display the absolute distance from the material origin.
Guides can also be added and other edits made by right clicking on the Guideline which will bring up the Guide Properties form:
The exact position can be specified by entering a New Position.
Guides can be given an angle by either entering an angle into the New Angle box or dragging the slider and clicking . Angles are measured in degrees counterclockwise from the x-axis. From an angled guide you can only create relative parallel guides.
Guide lines can be locked in position to stop them from being inadvertently moved by ticking the Lock Guide option.
Additional Guide Lines can be added that are positioned using absolute or incremental coordinates. Enter the Absolute or relative positions and Click .
Guides can quickly be toggled visible / invisible by clicking in the Top Left Corner of the 2D view:
Alternatively the visibility can be changed using View Menu ► Guide Lines from the Main MenuView Menu ► Guide Lines ► Delete All Guides from the Main Menu
Snapping Options
These options can be used to help create and edit vector geometry.
The Snapping Options form can be accessed by selecting Edit ► Snap Options from the Main MenuF4.
Display Text at Cursor
Displays the XY coordinates on the cursor making it easy to see the position for each point
Snap to Guides
When this option is checked ✓ drawing and positioning vectors will snap onto any horizontal or vertical guide lines visible in the 2D view.
Snap Guides to Geometry
When checked, ✓ the Guide Lines can snap to Geometry while being dragged.
Snap to Grid
Displays a grid of points separated by the Grid Spacing which can be snapped to when drawing or editing vectors and other objects in the 2D View.
Snap Distances
Snap to fixed lengths based on your zoom level. This occurs when creating shapes, dragging nodes or vectors.
Snap to Job Center and Corners
Snap to the job corners and center. This, also, control the job smart snapping
Fixed Nudge Distances
Objects can be moved small, fixed distances (nudged) by holding Ctrl + Shift and tapping the arrow keys. The Fixed Nudge Distance specifies the distance to move selected objects with each nudge.
Snapping Radius
The snap radius (pixels) will adjust how close the cursor must get to vector geometry in order to snap it. If you work quickly and grab and throw geometry at speed, you may prefer a larger Snapping Radius to pick up geometry that is vaguely near the mouse. If you work precisely or have complex overlapping geometry, you may prefer a smaller Snapping Radius to avoid having to zoom in to select one geometry in an area that has many nearby vectors.
Geometry Snapping
Used to control the position at which the cursor will snap when drawing and moving objects. When drawing, the cursor will snap to items on vector geometry depending what options you have selected in the form under this section.
Object centers, Span End points, Span Mid-points, Arc centers, intersections Horizontally, Vertically and the specified Angle and Distance Guide lines and the intersection of Guides
Smart Snapping
Smart snapping works by snapping the cursor to imaginary lines related to vectors and/or nodes. These lines will appear as dashed, and sometimes coloured, lines that go through the vector or node and the cursor point. You can snap to the intersection of those lines by hovering over the nodes that you're interested in. This reduces the need to create construction geometry (for example, for aligning nodes or vectors), and can be used in almost all the shape creation tools, node editing and transforming vectors.
Note
A node is the start, middle, or end point of a span.
Note
The snapping system is watching to see which vectors you hover the mouse over. It remembers that last few vectors as the ones you want to work with and draws the snap lines for those as a priority. There is a maximum number of nodes and vectors that can be "woken up" at the same time to avoid too many snap lines appearing at once.
Snapping lines can be drawn from:
- Nodes that were woken up by hovering the mouse over them or their span
- Vector properties, such as their bounding box or center point
- Material properties, such as extensions from the edge and the middle
Note
It is possible to wake up vectors on the other side of a double-sided job.
Cursor | Type | Description |
---|---|---|
Object Bounds | The theoretical bounding box surrounding the active vector | |
Horizontal and Vertical Lines | Horizontal and vertical lines passing through a node or a span midpoint. | |
Tangents | Tangents originating from a node or a span midpoint. | |
Perpendicular to Tangents | Lines which are perpendicular to tangents from nodes or span midpoints. | |
Connecting Lines | Lines connecting two nodes. Includes mid-point. | |
Span Geometry | Snap to the geometry of the vector. | |
Angular Constraints | Snapping to specific angles, as defined in the snap options F4. | |
Job | Horizontal and vertical lines through the center of the job. |
Object Bounds
These snap lines appear on the bounding box edges of the vector, and in the middle horizontally and vertically.
Vertical and Horizontal Lines
Nodes
The snap lines appear when the cursor is near the horizontal or vertical line passing through the woken nodes.
Vectors
Snap lines become available while moving vectors so that it is used for aligning them with other vectors.
Tangents
These snap lines originate from the woken node and will appear as an extension along the end of the belonging span.
Perpendicular to Tangents
These snap lines will be 90° from the tangent snap line.
Connecting Lines
If you wake two or more nodes, you could snap to the line connecting them. You could, also, snap to the mid-point of that line.
Span Geometry
This allows you to snap to the geometry of the vectors.
Angular Constraints
Job Edges & Centre
If you have the job snapping enabled, you could snap to the horizontal and vertical middle lines. This also includes the lines extending from the job's edges.
End point alignment
The start and end points can be aligned horizontally or vertically while the vector is being rotated.
Toolbar Snapping Options
Geometry Snapping, Smart Snapping and Grid Snapping can be switched on and off from the View Toolbar
Any change to the snap settings F4, through the Main Menu or the toggles on View Toolbar will be remembered for subsequent sessions.
Disable snapping temporarily
Snapping can be temporarily disabled by holding down the Shift key.
Edit
Undo | Steps backwards through the last 5 changes made by the user. | |
Redo | Steps forward through design steps that have been Undone using the Undo command (see above) to get back to stage that the user started using the Undo function. | |
Cut | Removes the selected objects from the job and places them onto the clipboard. | |
Copy | Copies selected objects to the clipboard, leaving the original in place | |
Paste | Pastes the contents of the Clipboard into the model (see cut and copy above). | |
| Delete | Deletes the selected object - same as hitting the Delete key on your keyboard |
| Selection► | Select various types of vectors |
| Align Selected Objects ► | Give the user all the options covered under the Align Objects section of the menu. Opens the Alignment Tools form. |
| Join Vectors | Joins open vectors. Opens the Join Vectors form. |
| Curve Fit Vectors | Allows arcs, Bezier curves or lines to be fitted to existing vectors to 'smooth' them. Opens the Fit Curves to Vectors form. |
| Nest Selected Vectors | Opens the Nesting form. |
Job Size and Position | Opens the Job Setup form. | |
| Notes | Opens a text box where you can record notes regarding this job, such as customer name, material required, special setup instructions or any other relevant text information you would like to keep when you save the job. If the text starts with a period/full stop/dot '.' , the Notes dialog will be displayed automatically each time the file is opened. The text from the Notes dialog can also be optionally output into the toolpath as a comment field. See the Post-Processor Editing Guide. |
| Document Variables | Opens the Document Variables dialog. |
| Snap Options | Opens the Snap Options dialog. |
| Options | Opens the Program Options dialog to allow the customization of certain aspects of the program. |
Selection
| Select All Vectors | Selects all the currently visible vectors in the Design (vectors on invisible layers are not selected). |
| Select All Open Vectors | Selects all the currently visible Open vectors in the Design |
| Select All Duplicate Vectors | Selects all the currently visible Duplicate vectors in the part - these are vectors which are exact copies of each other in terms of shape and location so that visually they appear to be only one vector. These can cause problems for some toolpath and modeling functions so it can be useful to delete them or move them to a new layer. |
| Select All Vectors On Current Layer | Selects all the vectors on the selected layer. |
| Unselect All | Deselects all the currently selected vectors in the part |
| Vector Selector... | Opens the Vector Selector dialog. |
Notes
- 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 / Close Vector with a Straight Line
Join with a Line finds the closest end points on 2 selected, open vectors and joins with a straight line. Close with a Line closes a single open vector with a straight line between its two end points.
Grouping and Ungrouping
Grouping objects allows you to select, move and manipulate them as if they were one entity. The process is entirely reversible by Ungrouping.
See Grouping and UnGrouping.
Edit Toolpath
This option is used to modify an existing toolpath. Click to select a toolpath in the list then click the edit option to open the form.
The vectors associated with each toolpath are automatically remembered, so editing a toolpath will automatically select the vectors in the 2D window.
Make the required changes to the toolpath parameters Click the Calculate button to update the toolpath
A toolpath can also be edited by double-clicking on its name in the toolpath list.
Overlap Vectors
Selected closed vectors that overlap can be merged together to create a new shape. These tools consider the closed vectors to be solid areas.
The following examples begin with these five vector shapes where the rectangle was selected last.
Only areas of the first selected parts (the circles) that are covered by the last selected vector (the rectangle) remain after this operation.
Component Tree
The model that you see in the 3D View is the result of progressively combining all of the visible components from the bottom of the Component Tree, to the top. The resulting model is known as the Composite Model. The order in which components are combined can have a significant impact on the final shape of the composite model and so you will often need to move components relative to one another within the Component Tree in order to achieve the end result you are intending.
For more information, see the 3D Design and Management page.
Combine Modes
To help you understand how the components are being combined, each component in the tree has an icon indicating how it is currently being combined with the components below
Grouping
Grouped components are also indicated by their own icon and the presence of a plus or minus control to the left of the visibility checkbox. These controls allow you expand or collapse the group to show or hide the group contents, respectively.
Every component exists on a single Level. These levels can be used to organize your modelling process. During the compositing process the contents of a level are combined first before the levels themselves are combined together.
Selection
Components can be selected in 3 ways:
- By left-clicking on the component's name in the Component Tree
- By left-clicking on the associated grayscale component preview image in the 2D view
- By double left-clicking directly on the component in the 3D view
In all cases, the new selection will subsequently be reflected in all three locations. So, for example, selecting a component in the Component Tree will simultaneously cause the associated 2D component preview to become selected in the 2D View, and the same component to become highlighted in red (or green if the selected component is obscured by another component) in the 3D View.
There are, however, some minor differences between the three methods of selection. Also, depending on the circumstances, there may be some advantages to selecting your components using one method rather than another.
Selection in the Component Tree
The component tree works in a similar way to the Window's file explorer. To select a component, simply click on it. To select multiple components, hold down a Ctrl key while clicking on each component you wish to add to the selection. While in this mode, clicking on a component that is already selected will cause it to be removed from the selection.
Pressing a Shift key allows you to select a range of components. Click on the first component in the range to select it, then holding a Shift key and pressing the last component you want selected will select all the components between the first and last selection.
Double-clicking a component or level in the Component Tree will automatically open the Component Properties tool - see the Component Properties section for more information on how to use this tool to modify the selected components.
Right-clicking an unselected component in the Component Tree will select it, and open its pop-up menu of related commands. Any commands you select will apply to this selected component only.
Right-clicking a component that is already selected, and is also one of several selected components, will open a similar pop-up menu of commands. Any commands you select from this menu will apply to all of the currently selected components.
Selection in the 2D View
The 2D component previews behave exactly the same way as vectors or bitmaps. They can be selected by a single, left-click. Several component previews can also be 'shift selected' (see above). Clicking on selected component previews again activates their interactive transform handles. These can be used to move, rotate or stretch the 2D component preview and its associated 3D component.
Selection in the 3D View
Because the left mouse button is used for twiddling the 3D view itself, a single left-click cannot be used for component selection directly. However, VCarve Desktop'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.
Editing in the 3D View
Many of the dynamic component editing tools can now be accessed directly from the 3D View. Editing the components in the 3D View makes it quick and easy to see the immediate effect of the changes to the Composite Model. To access these editing options a component or components must first be selected. Once selected then either clicking the component again in the 3D view or clicking the Transform Mode icon (Move, Scale, Rotate Selection) will activate the 3D Transform Handles. These take the form of solid and hollow blue squares around the component/s in the 3D View.
The majority of these will function in the same way that they do with objects in the 2D View. The additional larger solid blue square below the middle of the bottom edge of the model can be left-clicked to open a floating form that allows access to some of the components properties. This form can be moved if it is covering an important area of the job. From this form you can adjust the Combine Mode, Shape Height, Base Height, Fade and Tilt for the selected component/s. If you edit Fade or Tilt using this form, then when you click the Set button you must click the positions for this in the 3D View.
Position in the Component Tree
The position of the component in the Component Tree may affect the resulting combined model. This position can be altered by selecting one or more component(s) and clicking one of the buttons with a blue arrow at the top of the Component Tree. Alternatively, component(s) can be selected and dragged in component tree via mouse. If Ctrl is held when component is being dragged, then the component itself will not be moved, but it will be copied instead and placed at the desired location.
Group Selected Objects
Vectors can be Grouped allowing any number of vectors to be included as a single object that can easily be selected, moved and scaled etc. The Shortcut key for this operation is G.
Grouping vectors is particularly useful for machining purposes, where different vectors will be used for a single toolpath operation. Clicking any member of the group will select the entire group.
Draw Ellipse
Ellipse / ovals can be created interactively with the cursor and Quick Keys or by entering the exact coordinates for the center point, height and width with typed input.
Note
Pressing the Space-bar re-opens the last vector creation form you used. This is very useful when using other forms in between each shape you create.
Interactive - Cursor
The quickest and simplest way to draw an ellipse is:
- Click and drag the left mouse button in the 2D View to begin drawing the ellipse from its corner.
- While holding the left mouse button, drag to the required size.
- Releasing the left mouse button.
- Holding Alt and dragging creates an ellipse from the middle point.
- Holding Ctrl and dragging creates a circle.
Quick Keys
Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.
- Left-click and drag out your shape in the 2D View.
- With the left mouse button still pressed, enter a quick key sequence detailed below.
- Release the left mouse button.
Default
By default, two values separated by a comma, will be used to set width and height of your ellipse. One value will create a circle with the given diameter. While you are dragging out the ellipse, type Width Value , Height Value Enter or Diameter , Enter to create an ellipse with the specified dimensions.
Specifying Further Properties
By using specific letter keys after your value, you can also indicate precisely which property it relates to.
- Value X - Creates an ellipse at current dragged height but with set width
- Value Y - Creates and ellipse at current dragged width but set height
- Value W Value H - Creates an ellipse with set width and height
Examples
- 1 x Current dragged height with width (X) of 1
- 1 y Current dragged width and height (Y) of 1.
Exact Size
Accurate ellipses can also be drawn by entering the required XY origin point with the Width and Height of the oval. Click to create the ellipse.
Editing an Ellipse
To edit an existing ellipse:
- Select the ellipse to modify and open the Draw Ellipse form.
- The selected shape is displayed as a dotted magenta line.
- Edit the Width and Height values.
- Click to update the ellipse.
To modify another ellipse without closing the form hold a Shift key down and select the next ellipse.
Object Selection Tools
Once vectors have been created within VCarve Desktop or have been imported from other design software packages you may want to make changes to them. These changes may be to prepare for machining or for use as construction vectors for making 3D shapes using the Modeling Tools. There are a number of functions for editing vectors which will be covered in this section of the manual. All the icons under the Edit Vectors section of the Drawing Tab will be referenced along with the icons under the Align Objects section of the menu.
Editing Modes
From the 2D view a vector can be selected and then three different editing modes allow different dynamic edits to be made to the vector(s) depending on which option is selected from the Edit Vectors section.
The three editing modes are:
By default the software is normally in the Vector Selection mode.
Crop Bitmap
Select the image you would like to crop. Then using shift + left click select the closed vectors you would like to use to crop the image. You may select multiple vectors but the image must be selected first. Click the crop bitmap button to clear the image outside of the vector. If multiple vectors are used for the cropping then the crop tool leaves only the area of the image that lies inside the selected contours.
Document Variables
Document Variables provide a mechanism for defining values that can be used in VCarve Desktop's Document Variables. They can either be created in the Document Variables dialog which is accessible under the Edit menu, or created from any Calculation Edit Box which supports variables by right clicking and selecting Insert New Document Variable from the Popup Menu.
Naming Document Variables
New Document Variable names must begin with a letter and then may consist of letter, number and underscore characters. Once created, they may be edited in the table beneath the New Variable section of the Document Variables Dialog.
Variables can be exported to a text file and imported into another job. When importing, any existing variable values with the same name will be replaced.
Deleting Document Variables
Variables may be deleted if they're not being used in any toolpath calculations but only when there are no toolpath creation forms open.
Using Document Variables
Once created a Document Variable may be used in any Calculation Edit Box by enclosing its name within a pair of curly braces as illustrated in the figure below.
Right clicking in a Calculation Edit Box provides a Popup Menu that provides shortcuts for creating new Variables and inserting existing variables into the Edit Box.
Once a Document Variable has been created from the Popup Menu it will be inserted into the Edit Box.
Accessing Document Variables
Declared Document Variables can be easily accessed from a calculation edit box. Right-click on the calculation edit box and you will be presented with a menu showing the document variables available currently, as well as an option to quickly insert a new document variable.
Set Size
Selected items in the 2D View can be accurately scaled or resized using this option.
Mode
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.
Anchor
The anchor position determines the point on your selected object's bounding box that will be resized to the dimensions entered.
Link XY
Checking ✓ this option will always scale the height and width in proportion. Leaving the Link option unchecked allows non-proportional scaling
Auto Scale Z
This option sets a specific mode of scaling for 3D Components. When it's checked, ✓ scaling a model component in X or Y will result in it also scaling proportionately in Z, as such if you increase its size in X and/or Y then its Z Height will also increase and conversely when you reduce its X and/or Y size it will shrink in height. When it is unchecked then the Z Height of your Components will remain constant regardless of any X and/or Y scaling done either within this form or dynamically using the mouse in the 2D or 3D View.
Interactive Sizing
The default mode is to enable selected items to be scaled interactively by clicking twice with the mouse.
The process is:
- Select the vectors
- Click a second time to activate the interactive options - handles on the selection box
- Click and drag on the white handles
The keyboard shortcut T opens the Scale form in interactive mode
Scale Model Height
This tool applies a global scaling to your final composite model. This allows you to accurately fit a design within the available material or to manage the depth of cuts required, without having to individually adjust the depth of each of the contributing Components.
Scale Both Sides
This option can only be selected when working within a 2 Sided Setup. Checking ✓ this option enables you to scale both sides of the model. If this is unchecked then you are only scaling the model of the side you are currently working on.
Scale Height
This slider will allow the user to increase and decrease the height of the model as a percentage based on its original height (when the Scale tool was selected).
Set Exact Height...
Clicking button lets the user define a specific value (in the current working units) for the height of the model, rather than use the proportional slider. If you are working in a two sided environment you have the option scale both sides. Checking ✓ this option enables you to scale both sides of the model. If this is unchecked then you are only scaling the model of the side you are currently working on.
Apply/OK
Exits the dialog keeping the changes made to the Model.
Close/Cancel
Exits the dialog discarding the changes made to the Model.
Interface Overview
- The Main Menu Bar (the Drop Down Menus) along the top of the screen (File, Edit, Model, Toolpaths, View, Gadgets, Help) provides access to most of the commands available in the software, grouped by function. Click on any of the choices to show a Drop-Down list of the available commands.
- 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.
- 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.
- 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.
- The 3D View is where the composite model, toolpaths and the toolpath preview are displayed.
- If you wish to see the 2D and 3D views simultaneously, or you wish to switch your focus to the Toolpaths tab at a later stage of your design process, you can use the interface layout buttons (accessible in the 2D View Control section on the Drawing Tab) to toggle between the different preset interface layouts.
Managing the Interface
The tool pages have Auto-Hide / Show behavior which allows them to automatically close when not being used, thus maximizing your working screen area.
The software includes two default layouts, one for designing and one for machining, which can automatically and conveniently set the appropriate auto-hide behavior for each of the tools pages. Toggle layout buttons on each of the tools pages allow you to switch the interface as your focus naturally shifts from the design stage to the toolpathing stage of your project.
Accessing Auto-hidden tabs
If a tools page is auto-hidden (because it is currently unpinned, see pinning and unpinning tools pages, below), then it will only appear as a tab at the side of your screen. Move your mouse over these tabs to show the page temporarily. Once you have selected a tool from the page, it will automatically hide itself again.
Pinning and unpinning tools pages
The auto-hide behavior of each tools page can be controlled using the push-pin icons at the top right of the title area of each page.
Default layout for Design and Toolpaths
Aspire has two default tool page layouts that are designed to assist the usual workflow of design, followed by toolpath creation.
In all three of the tools tabs there are 'Switch Layout' buttons. In the Drawing and Modeling tabs, these buttons will shift the interface's focus to toolpath tasks by 'pinning-out' the Toolpaths tools tab, and 'unpinning' the Drawing and Modeling tools tabs. In the toolpaths tab, the button reverses the layout - unpinning the toolpaths page, and pinning-out the Drawing and Modeling pages.You can toggle between these two modes using the F11 and F12 shortcut keys.
Manual Machine Configuration
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.
- Having a machine configuration allows you specifiy different feeds and speeds for your tools in the Tool Database.
- And then it will allow you to easily select a machine to save your toolpaths with later on.
Thread Milling Toolpath
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.
Tool Selection
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
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.
Multi Point Tools
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.
Advantages and Disadvantages
- Single point tools have more flexibility when it comes to the threads that they can cut. The cutting paths can compress or extend to create threads with different pitches.
- Single point tools will be slower. They must machine all the threads with the one cutting edge, so will be many times slower than the equivalent multi-threaded tool.
- For large wood-working style jobs then it is unlikely that you will find multi-threaded tools of the right size.
- For cutting standard sized threads then a multi-threaded tool will be correctly spaced and easy to use.
- In the software, with a multi-point tool you cannot alter the pitch, and the toolpaths thread length must be at most the thread length of the tool.
Thread Definition
Pitch Preset
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.
Pitch
The Pitch describes the difference between the ridges of the thread.
Diameter
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.
Fit Tolerance
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.
Create Circles for Internal Threads
When cutting an internal thread you may have an area inside that thread that needs to be removed with another tool. Calculating what area can be safely removed can be a little bit of work, so to make that easier the button will create a circle that the user can apply a Pocket toolpath to, to clear this region.
Thread Type
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.
Direction
Thread Direction
A thread can be either right-handed or left-handed. This determines the clockwise/anti-clockwise direction of the thread as it spirals.
Cut Direction
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.
Created Threads
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:
Use Vector Selection Order
If this option is checked, ✓ the vectors will be machined in the order you selected them. If the option is not checked the program will optimize the order to reduce machining time.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Draw Curve
This tool creates a smooth, flowing, continuous curve through clicked points.
Form
Draw Curve does not require an associated form, just use the mouse cursor directly within the 2D View.
Controls
- Click in the 2D View to begin drawing at the clicked point.
- Move the mouse pointer within the 2D View and click the left button to insert as many points as you require. A curve will be created that smoothly joins your points.
- Click the right mouse button or press Esc to finish drawing your curve and close the tool.
- Alternatively, press Space Bar to finish drawing one curve, but keep the tool active so that you can immediately begin drawing another curve.
Left Clicking
Left clicking when the mouse pointer is close to the first point on the curve will snap the curve closed.
Extending Contours
An existing open contour can be extended by holding down the Ctrl key and then clicking on either its start or end point.
CTRL clicking on the start point of a contour will cause the contour to be reversed before extending.
Delete Toolpath
This tool is used to delete calculated toolpaths from the Toolpath List. Simply select the toolpath to be deleted and click the Delete Toolpath button to remove it.
Alternatively, you can delete one or multiple toolpaths in the Toolpath List by right mouse clicking on a toolpath. Then from the drop-down menu click on the Delete option. This will present the options as shown in the image: Delete This, Delete All Invisible, Delete All Visible, Delete All.
Delete This will delete just the toolpath whose name you right mouse clicked on.
Delete All Invisible will delete any toolpaths in your Toolpath List that do not have a check-mark ✓ next to their name and are therefore currently not visible in the 2D or 3D Views.
Delete All Visible will delete any toolpaths in your Toolpath List that have a check-mark ✓ next to their name and are therefore currently visible in the 2D or 3D Views.
Delete All will delete all the toolpaths in your Toolpath List.
If you have incorrectly deleted a toolpath (or multiple toolpaths) then you have the option to Undo the toolpath(s) deletion via the Undo command on the Edit drop-down menu, the Undo icon on the Drawing Tab or the Undo shortcut key combination Ctrl + Z.
Mirror
Selected vectors/bitmaps/component grayscale previews can be mirrored to a new orientation.
Selected objects can also be mirrored about axes of symmetry relative to the bounding box of the selection, using the standard options on the Mirror Form.
- Select the object or objects to mirror.
- Click on the Mirror icon to open the Mirror Form.
- Select the Create a mirrored copy option to leave the selection and create a new set of objects.
- Click the button to accept the changes.
Use Rotated Bounds
This option is available only when a single object is selected. When it's checked, it will flip the object around its local rotated bounds as shown in the Selection Tool. If the object isn't rotated, it will just operate normally.
Flip About Line
Select the Vector to mirror, and hold Shift and then select the Line vector you wish to use as the mirror. This option then becomes available to select and will flip the desired vector across the Mirroring Vector.
Shortcuts
The following shortcuts can be:
- H - Mirror Horizontally
- Ctrl + H - Create mirror. Copy Horizontally
- Shift + H - Mirror horizontally around center of material
- Ctrl + Shift + H - Create mirror copy horizontally around center of material.
- V - Mirror vertically
- Ctrl + V - Create mirror. Copy Vertically
- Shift + V - Mirror vertically around center of material
- Ctrl + Shift + V - Create mirror copy vertically around center of material.
Layer Management
Vectors, Bitmaps and Component Grayscale's can be assigned to different layers.
All the objects assigned to a layer can then be simultaneously selected, labeled, colored, temporarily hidden or even locked (to prevent accidental editing) using the Layer Management tools. Even for relatively simple designs, organizing the elements of your artwork onto layers can make managing your project much easier.
The Layers Tab
To get a complete overview of the current layer structure of your artwork while you are working, or to carry out more extensive organization of the layers, you can also use the Layers tab. The Layer List is identical in both the Layer Control and the Layers tab, but the latter can control layer ordering and be left visible, pinned or even undocked, while you continue to work on the artwork itself
List Item Command and Icons
Each layer in the list has five elements:
Status Icon
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 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.
Add New Layer
New Layers can be added using the Add New Layer button. Alternatively a new layer can be created directly from the 2D View by right-clicking an object and selecting either the Copy to Layer ► New Layer... or Move to Layer ► New Layer...
Layer Name
It is always preferable to take the opportunity at this stage to give your new layer a meaningful name relating to its content or purpose. Later on this name will make it easier for you to manage your layers as your design becomes more complicated
Drawing Color
All the vectors on this layer will be colored according to this setting. This can be a very useful way of distinguishing between the vectors that are on different layers, directly in the 2D View.
New Layer is Visible
With this option checked, ✓ the new layer will automatically be visible as soon as it is created.
New Layer is Active
With this option checked, ✓ the new layer will automatically become the active layer and any subsequent vector creation or manipulation will occur on this new layer.
Insert New Layer
An even quicker way to add new layers is via the Insert Layer command from a layer's right-click Pop-Up Menu. This command will create a new layer above the selected layer which will be visible, unlocked and colored black. After creation the new layer item's name is ready to be immediately edited by typing a new name in.
Moving Objects to Layers
Objects on any layer can be moved onto another layer by right-clicking the object in the 2D View and selecting Move to Layer from the pop-up menu. It is also possible to place a copy of selected object to another layer by selecting Copy to Layer from the pop-up menu.
Draw Polygon
Polygons (e.g. Triangles, Pentagons, Hexagons etc.) can be created interactively with the cursor and Quick Keys or by entering the number of sides, exact coordinates and radius using typed input.
Interactive Creation
The quickest and easiest way to draw a polygon is by using the mouse in the 2D View.
- Click and hold the left mouse button to indicate the center point.
- Drag the mouse while holding down the left mouse to required radius.
- Release the left mouse button to complete the shape.
Note
Holding ALT and dragging creates a polygon from the middle point.
Quick Keys
Instead of releasing the left mouse button when you have dragged your shape to the required size, you can also type exact values during the dragging process and set properties precisely.
- Left-click and drag out your shape in the 2D View.
- With the left mouse button still pressed, enter a quick key sequence detailed below.
- Release the left mouse button.
Default
By default, entering a single values will be used to set the radius of your polygon. While you are dragging out the polygon, type Radius Value Enter to create a polygon with the precisely specified radius.
Example
- 2 . 5 Enter - Creates a polygon with a radius of 2.5. All other settings as per the form
Specifying Further Properties
By using specific letter keys after your value, you can also indicate precisely which property it relates to.
- Value D - Creates a polygon with the diameter specified, with all other properties as per the form.
- Value S Value R - Create a polygon with the specified number of sides (S) and the outer radius (R)
- Value S Value D - Creates a polygon with the specified number of sides (S) and the outer diameter (D)
Examples
- 1 R - Outer radius 1, number of sides as per form
- 1 D - Outer diameter 1, number of sides as per form
- 8 S 1 R - An 8 sided polygon with outer radius R of 1
- 6 S 2 . 5 D - A 6 sided polyon with an outer diameter of 2.5
Exact Size
Polygons can also be drawn by entering the required XY origin , selecting either Radius or Diameter and entering the required size.
Click to update the circle
Editing Existing Polygons
To edit an existing polygon select the polygon, edit the parameters and click to update the circle.
Right Mouse Click Menu
Clicking the ►RIGHT hand mouse button in different places in VCarve Desktop will display a menu with choices which depend on the area of the software being clicked on and/or the object or selection that the mouse cursor is positioned over. This page details some of these areas and the menus that you will see when RIGHT mouse clicking.
2D View
This menu is displayed when you Right mouse click in 2D View either in the white background of the part or over a selected vector. Most of these options repeat functions and icons described elsewhere in this manual, you should refer to the appropriate section to view how these work.
Layer and Side Operations
The Copy to Layer, Move to Layer, Move to Sheet, Copy to other Side, and Move to other Side options are unique to this Right click menu.
- Copy to Layer allows you to copy an object onto an existing Layer or to create a New one to copy it onto.
- Move to Layer gives you the same choices but moves the original object rather than making a copy.
- Move to Sheet can only be used if you have generated additional Sheets through the Nesting process, in that case it allows you to move objects from one Sheet to a different one from the list available.
- Copy to Other Side copies the selected objects onto the other side in a two-sided job. The objects will be transformed so that they match up when looking through the material.
- Move to Other Side moves the selection similarly to the Copy operation.
Span Editing Menu
If the current selection mode is set to Node Editing, one of two different menus will appear when the user clicks the RIGHT mouse button depending on whether the cursor is currently over a vector Node or a Span of a selected vector in the 2D View.
These menus have functions in them that correspond specifically to this selection and position. The menu shown here will appear when the cursor is over a Span of a vector in Node editing mode.
You can see a variety of choices:
- 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.
Node Editing Menu
This menu will appear when the cursor is over a Node of a vector in Node editing mode.
You can see a variety of choices:
- Delete the Point
- Smooth it
- Insert a point at a virtual midpoint
- Cut the vector at that point
- Change the point to be the Start Point of the vector or extend the vector using the Polyline tool.
- Horizontal or vertical mirror mode for node editing can be toggled on or off.
From this menu you can also close any selected open vectors, Join two selected open vectors, Exit node editing mode or lastly see and edit the exact XY co-ordinate position of the node by selecting Properties.
Many of these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the keyboard when the mouse is in position (over a node-edit vector node) instead of Right Clicking the mouse button to access the menu.
Bitmap Properties Dialog
When a Bitmap or Component Grayscale is the selected item in the 2D View and the RIGHT Mouse menu is activated then there will be an additional option in the pop-up menu called Object Properties. This will open the dialog shown below which can be used to fade the Bitmap or Grayscale object strengthen or fade the detail in it when it is not selected. This can be helpful to make it easier to see features perhaps to help you manually trace vectors over it or to fade them so its easier to see vectors that overlap the object.
Level 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.
Component Menu
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.
Component Grayscale Menu
When a Component Grayscale is the selected item and Object Properties is selected it opens the Bitmap Properties slider, allowing you to change the fading of the grayscale component. Two other options are also available on the Right mouse click menu for a selected Component Grayscale. Move to Front and Move to Back. Clicking Move to Front will make the selected Grayscale appear over all the other Grayscales on the same layer so you can see the selected one more easily. Move to Back will send the selected one behind all the others on the same layer so that it is easier to see all the other Grayscales in the part.
3D View Menu - Selected Component
When a component(s) is selected in the 3D view you can RIGHT mouse click and make changes to that selected component(s). You can check the combine mode of a component. You can Unselect a single component or Unselect All depending on how many components you have currently selected. You can hide and delete a component. You can open up the properties form for that component and you have the option to move the selected component(s) to an existing or new Level.
If you choose New Level you will be presented with the box below, where you simply add in the name for the new level and choose a combine mode from the dropdown menu.
3D View Menu - Non-Selected Components
When you RIGHT click on a component without selecting it first the menu will display the names of the components that are positioned at the point your cursor is within the job space. Selecting the name of the component will select it and open up the Properties form for that selected component.
Clipart Menu
When you RIGHT click on a piece of clipart in the clipart tab you have the option to import it to a new or existing level in your job. This will position the object in the center of the workspace and add it to the top of the list of Components on the selected Level or if you choose New Level will allow you to enter a name and Combine Mode.
Toolpath List Menu
When you RIGHT click on a toolpath name within the Toolpath List there are various options you are presented with to alter this toolpath. You can show a toolpath where you have the option to
- Show This,
- Show Only This,
- Show All But This
- 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.
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.
Offset Vectors
Selected vectors (open or closed) can be offset either inwards or outwards to create new vector shapes that might be useful for edge patterns or borders etc. To offset a vector shape, use the following steps:
- Select the vectors to offset
- Select the required direction - Outwards / Right or Inwards / Left
- Enter the Distance
- Click the button
Options
The offsetting options are slightly different in their behavior depending on whether the vector to be offset is open or closed. See below for more information.
Create sharp offset corners
Will retain any sharp corners in a design.
Offsetting Open Vectors
When offsetting open shapes, the options are either to the Right or Left side of the selection. The direction of open vector(s) is very important as this is used to decide the right and left side of the selection. Selecting Node Edit mode (pressing N on the keyboard) will display a Green node at the start of the vector. Looking along the vector(s) from the green node indicates the direction and the image below shows offsets to the left and right of an open vector.
Positioning an Imported Model
Zero Plane Position In Model
This slider bar determines where the 3D model will be cut-off when converting to a Component. You can move this up and down with the mouse or use the Middle or Bottom buttons to locate the plane in the correct position.
Note
Anything in the original model which is an undercut (goes underneath another part of the 3D model) will be discarded and a vertical wall will be created down to the plane from the silhouette (looking down Z axis) edge of the model.
Create both sides
If you are working in a 2 sided setup you can check ✓ this option and two components will be created - one looking down the Z axis from above to the zero plane and one looking up from below. Each side of the model will go onto a side. This will provide you with the geometry that can be edited to cut the original imported 3D part as a 2-sided job.
If you were importing a model that contains a non-convex surface for instance a bowl you can import the entire model on each side by sliding the slicing plane all the way to the bottom.
Discard data below zero plane
Checking ✓ this will remove any data below the original Zero level within the imported 3D model. If the model is effectively a negative model such as a dished or recessed design with a flat plane then you should uncheck this option to make sure you retain the 3D data below the plane.
Highlight Undercuts
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".
Back, Cancel and Import
The final options are:
- will return you to the Import 3D Model > Transform form.
- will close the Import form and not import your model.
- with complete the process and convert your 3D model into a 3D Component within VCarve Desktop
License Registration
If you have recently purchased your machine which came with some licencse details for VCarve Desktop (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 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 which will take you the License Dialog.
If you click the button, you can continue to use your software but will be prompted again to complete the registration process.
Job Setup - Double Sided
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.
In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.
Job Type
Single Sided job type should be used when design only requires the material to be cut from one side. This is the simplest type of job to design and machine.
Double Sided Job type is useful when it is desired to cut both sides of your material. Aspire allows you to visualise and manage the creation and cutting process of both sides of your design within a single project file.
Rotary job type enables the use of a rotary axis (also called a 4th axis or indexer).Aspire will provide alternative visualisation, simulation and tools appropriate for rotary designs.
Job Size
This section of the form defines the dimensions of the material block you will be using for your project in terms of width (along the X axis), height (along the Y axis) and thickness (along the Z axis).
It also allows you to select which units of measurement you prefer to design in - either inches (Imperial/English) or millimeters (Metric).
VCarve Desktop only supports job sizes up to a maximum of 25 inches square without tiling.
You can cut jobs larger than this limit but you will need to use the Toolpath Tiling feature to cut the job in sections.
Z Zero Position
Indicates whether the tip of the tool is set off the surface of the material (as shown in the diagram) or off the bed / table of the machine for Z = 0.0.
Zero off same side
This option allows Z Zero to reference the same physical location, regardless whether material is flipped or not
XY Datum Position
This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's position.
Use Offset
This option allows the datum position to be set to a value other than X0, Y0.
Flip Direction Between Sides
This section gives choice between horizontal and vertical flipping when changing machining side. Aspire uses that information to correctly manage the alignment of the geometry relating to each side.
Design Scaling
When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click
Modeling Resolution
This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.
As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.
The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.
As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.
Appearance
Clicking will pop up a dialog allowing you to set the color or material effect which will be applied to the base 3D model. It is possible to change this at any time and also to apply different colors and materials to different Components using the Component manager. See Preview Toolpaths to learn more about different material settings and adding custom material effects.
Join / Close Vector with a Smooth Curve
Join with a Curve finds the closest end points on 2 selected, open vectors and joins them together with a smooth curve.
VCarve Desktop has two smooth joining methods:
- A smoother method (new for V9.5)
- A more symmetrical shallower join method
Copy Along Vectors
This tool automatically creates repeating patterns of objects by placing copies of them along the length of one or more selected vectors. The tool allows any existing object to be used but it also has an option specifically for the creation of circles, which is a common design element for patterns of this sort.
Copy Object
Any shape vector or group of vectors can be copied along a curve or curves. The first vector or group of vectors selected is the object that gets copied multiple times along the curves.
Copy Circles
Enter the diameter of the required circles
Distance between copies
This is the distance along the selected curve between each pasted vector. The Force even spacing option ensures that objects are pasted at the end points on the curve(s). If this option is not selected the pasted objects will be placed at the specified distance and may not match the exact length of the curve.
Number of copies
Selecting a specific number of copies automatically sets the specified number of copies along the entire length with an even spacing between them
Align Objects to curve
With this option selected the pasted objects are automatically aligned 'normal' or perpendicular to the curve they are being copied onto. If this is not selected, the copied objects stay in the orientation of the original.
Create Copies on new layer
This option creates the multiple copies on a new layer making it much easier to select and organize the resulting vectors for machining purposes etc.
Reverse Direction
If your copies appear upside down, this option will perform the copy operation in the opposite direction along the selected vectors and the resulting copied shapes will be created the other way up.
Post-Processor Change Log
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.
Vector Selector
This tool allows you to easily select vectors which meet a set of criteria, such as open, closed, circular and also matching constraints based on layers. The dialog can be accessed from the Edit ► Vector Selector menu item, or from the button on each toolpath form. When the command is executed the dialog shown is displayed.
The dialog is used to configure a set of 'filters' that determine which vectors will be selected. A filter is enabled by clicking on its check box, or selecting a 'radio button' option, the current selection will be updated with all the objects in the file which match the current filter options.
Generally you will start at the top of the dialog and work downwards, specifying more and more explicit filters to determine the required selection exactly.
The simplest option is just to use the form to Select Closed Vectors in the job or Select Open vectors (you can specify both, in which case all vectors will be selected as long as they are on a visible layer).
The most common way to use the Vector Selector is to select all the vectors on a given layer as shown in the screenshot of the dialog below.
Note
When opened from Edit ►Vector Selector, the options Associate with toolpath and Set toolpath Cut Depth from imported vectors are not available. These options are only usable when applying the vector selector from a toolpath form.
Selection
The Selection: section at the top of the dialog is continuously updated to show the results of the current filter and the 2D view is also updated to show what is currently selected. The Objects: entry shows the total number of objects selected, if these objects include Text or Groups, this number may be less than the total of Closed and Open vectors displayed on the following line. For instance, a block of text is one object but will usually consist of many closed vectors. If a group contains both open and closed vectors, it will be selected as matching both Open and Closed filters.
Geometry Filters
The Geometry Filters section is used to specify constraints on the type of vectors to select. You can choose to select open vectors and/or closed vectors. Instead of selecting All Closed Vectors, the dialog can be used to select Only Circles and can even be used to specify an exact diameter and tolerance for the circles to be selected. This can be very useful for selecting vectors for drilling toolpaths, particularly if the vectors have not already been sorted into layers.
Layer Filter
The Layer Filter section allows you to pick one or more visible layers on which to select vectors which match the geometry filter. Alternatively, the All visible layers option disables the filtering by layer and selects all vectors which match the geometry filter regardless of the layer they are on, as long as that layer is visible.
Advanced Toolpath Templates
By associating a template with the result of a Vector Selector filter, we can make a template to automatically select the vectors it is intended to machine. A simple case would be to create a template which consisted of a Pocketing toolpath set up to machine all closed vectors on a layer called Pocket. After loading this template into a new job and choosing Toolpaths ► Recalculate All Toolpaths , the toolpath would be recalculated automatically selecting all closed vectors on the layer called Pocket.
The advanced templates are created by selecting the vectors for a toolpath using the Selector... button on the toolpath form. When a toolpath form is first opened, the Vector Selection: section on the form will show that vectors are being selected manually as shown below...
Pressing the Selector... button will display the Vector Selector form as shown previously. After making your geometry selection and before you close the form, select the Associate with toolpath option on the form as shown below.
After the Vector Selector form closes, the Toolpath form will indicate that Vector Selection is now 'Automatic' as shown below...
Note
Calculate the toolpath to apply the changes you have made.
When you re-calculate or edit a toolpath that has the Vector Selection mode set to automatic, the vectors which match the filter when the toolpath is re-calculated or edited will be selected. To cancel the Automatic vector selection mode, you can just select the vectors to machine normally with the mouse, or use the Selector... button to bring up the Vector Selectordialog again (the settings are remembered) and uncheck the Associate with toolpath option.
If toolpaths with the Vector Selection mode set to Automatic are saved as templates, these setting are saved with the template. When the template is re-opened and the toolpaths recalculated, they will automatically select all vectors which match the filters specified with the Vector Selector for that toolpath.
If you load a toolpath template which has toolpaths associated with layers which don't exist in the current file, the Missing Layers for Template dialog will be displayed. It lists all the missing layers and offers you the choice of having them created automatically, deleting toolpaths associated with missing layers or just loading the toolpaths as is.
Choosing to allow the dialog to automatically create the missing layers allows a toolpath template to be used to create 'standard' layers for machining operations and load the toolpaths ready to be calculated. All you then need to do is move vectors to the appropriate layers and recalculate all the toolpaths.
Choosing the Delete all toolpaths associated with missing layers option allows you to create a single template with many toolpaths and have the ones which aren't appropriate to the current job automatically deleted.
Options Dialog
Note
Many of the choices in this dialog will not take effect until the software has been exited and restarted.
Window Layout
Save Tab Layout | Save the layout and the 'pinned' state of the command and toolpath fly out tabs. |
Save Dialog Layout | Save the size, position and visibility for dialogs such as the Layer control and Toolpath Control dialogs. |
Save View Layout | Save the layout of the 2D and 3D view windows. |
Display Splash Screen | Display the program Splash Screen, while the program is loading. |
Top Side Ruler Color | The colour of the ruler on the top side in a two-sided project. |
Bottom Side Ruler Color | The colour of the ruler on the bottom side in a two-sided project. |
Tab location | Determines where handles for switching between tabs are located |
3D View Settings
Shaded Background Style | Allows to choose between Solid, Gradient and Image background styles. |
Background Color | Change the background color used for the 3D view. Used with Solid and Gradient background styles. |
Gradient Background Color | Change the bottom (lightest) color used for the 3D view. Used with Gradient background style. |
Draw Origin | Draw the origin arrows by default on startup. |
Draw Material Block | Draws Material Block boundaries by default on startup. |
Use Color Shaded View | Draw shaded model in 3D view by default on startup. |
Print 3D View Shaded Background | Include the shaded background when printing. |
Animate Camera Moves | Switch on/off animation in the 3D View when selecting View positon from the Iso View, Down X, Down Y or Down Z icons. |
Image File Path | Path to the image to be used as background. Used with Image background style. |
Use Software Renderer | If ‘Yes’ this option switches from hardware GPU rendering to Software rendering which instead utilises the CPU. Software rendering can be preferable in cases where there is limited GPU capability or there are compatibility issues. This will require a software restart for any changes to take effect. |
Anti - Aliasing mode | Anti-aliasing can improve the graphic resolution by preventing the distortions and artefacts within the rendering caused by two or more points becoming indistinguishable from one another. There are four different options for the level of anti aliasing you would like to apply; None, 2X,4X and 6X depending on the level required. |
Smooth Shading | Select ‘Yes’ to enable smooth shading in the rendering of components which will give them a smoother less faceted (many individual sides) appearance. Turning this feature on will utilize more graphics memory than when disabled. |
Toolpath Settings
Show Toolpath Operations with Preview | When the toolpath Preview form is visible, keep the 'Toolpath Operations' section visible (requires more screen space). |
Auto Open 3D view | Automatically swap to 3D view after calculating a toolpath. |
2D Solid Preview Color | Color used to draw the solid 2D toolpath preview with. |
Create 2D Previews | Create 2D previews of toolpaths in 2D view. |
Select Sheet When Edit Toolpaths | If a toolpath is associated with a sheet, select sheet when edit toolpath. |
Toolpath Geometry Fixing Timeout | Number of seconds the program will spend trying to fix problems with geometry when calculating toolpaths. |
Drop Tool | When projecting a toolpath onto the model, drop the tool on surface rather than project. If this is set, the toolpath will follow the surface of the model better, but could be slower to calculate. |
2D Toolpath Tolerance | Tolerance to apply to 2D toolpaths after calculating to reduce file size. |
3D Toolpath Tolerance | Tolerance to apply to 3D toolpaths after calculating to reduce file size. |
VCarve Toolpath Tolerance | Tolerance to apply to VCarve toolpaths after calculating to reduce file size. Note We strongly recommend that the Toolpath Tolerance should be left at their default settings unless different values are recommended by your machine tool manufacturer. If you do have a machine which struggles with the default settings, try doubling the values and cutting a test-piece to assess the tradeoff between machining times, file size and final machined quality. We have done some limited testing and on a sample complex 3D model, increasing the '3D Toolpath Tolerance' to 0.001 inches gave a 40% decrease in file size and no noticeable difference in quality on the test machine and job. In the test case there was no measurable difference in machining time on the CNC machine the test was carried out on. |
Maximum Toolpath Undo Stack Size (MB) | Maximum size in MB of Toolpath data undo stack for storing toolpath delete state. |
Append duplicated toolpath | When duplicating a toolpath, this determines whether it places the new toolpath next to the original or append it to the end of the list. |
Append new toolpaths to selected group | If a toolpath group is selected, add newly created toolpaths to the end of the selected group rather than to the end of the list. |
Use new raster | Generate raster toolpaths that are more consistent in regards to machining direction, even for complex shapes. |
Check depth of all toolpaths | If this is set to try then when job size changes are made then all toolpath depths are checked. If it is set to false then only the toolpaths which are visible have their depth checked |
Default toolpath filtering mode | Allows you to choose the toolpath filtering mode used when new file is created or opened. |
General Settings
Use Graphics tablet | Switch on support for graphics tablet drivers, if installed - for use with the sculpting tool. |
Process User Files | Enable/disable processing of files in the 'Vectric Files' folder in your common user document folder. |
Recent File List Size | This sets the maximum number of items that will be displayed in the Recently opened files... list in left hand side bar of the interface when there is no file currently loaded. The list will not increase in size until the software has been re-started and more files have been opened and/or saved. |
Recent Font List Size | Sets the maximum number of recently used fonts that will be listed at the top of the font selection box. |
Show the clipart Subfolder Contents | If set to Yes then this will show the contents within the selected Folder in the Clip Art browser along with up to 3 sub-folders if they exist and contain appropriate file types. If set to No it will only display the contents of the selected folder, not sub-folders. |
Always open local documentation | Force open the local copy of the documentation when accessed through the Help menu. VCarve Desktop automatically opens the local documentation if you have no internet connection or if the server is taking too long to respond. |
Smooth Join Vectors | Produce a smoother join between 2 vectors. This is option is there mainly to support older behavior. |
Default to last used text anchor position | Control the default location of the anchor when creating a text object. This is to either default it to the last set location, or always default to a specific location. |
File Dialog Default | This option controls the default directory that is opened when opening or saving files. The default Global options will open the last used folder as per the Operating Systems default behavior. If you choose Operation, the software will remember the last used folder for that particular operation. We divide operations in broad categories, such as, vector import / export, model import / export, toolpaths, tools, etc... If you choose Job, we will always default to your saved job's location. |
Confirmation Choices
Sheet Toolpath Deletion Check | When a sheet is deleted, you can choose whether the associated toolpaths will also be deleted. |
Toolpath Vector Intersections Check | If vector intersections are detected calculating a V-Carve or Pocket toolpath you can choose to be asked what to do next or to open the Vector Validator. Alternatively, you may forgo the intersections check entirely. |
Radiused Offset Intersections Check | If vector intersections are detected when performing a radiused offset you can choose to be asked what to do next or to open the Vector Validator. Alternatively, you may forgo the intersections check entirely. |
Sharp Offset Intersections Check | If vector intersections are detected when performing a sharp offset you can choose to be asked what to do next, to open the Vector Validator or to proceed with the offset anyway. |
Warn about unsuitable components for embossing | When attempting an embossing operation on a low relief component, display warning to indicate that this model may not be suitable. |
Ask which version of the tool database to download | When downloading a tool database from your portal, display a dialog to allow you to specify a database associated with a different product. Otherwise always download the database associated with the current product. |
Duplicate Toolpath
The Duplicate Toolpath option creates and adds a copy of the selected toolpath to the Toolpath List. An index number is automatically added to the name of the new toolpath. For example:
Cut out - 1/4 inch End Mill will create a copy with the name Cut out - 1/4 inch End Mill (1)
Copying externally generated 3D toolpaths (as, for example, from PhotoVCarve) will also create a duplicate grayscale thumbnail image in the 2D View, which can then be used to position the toolpath within your job.
View Toolbar
Above the view window is a handy toolbar that allows easier access to common tools. With the ability to create a double sided project you have easy access to switch between the Top and Bottom Sides of your project. The Layers Drop down bar has now moved from the drawing tab to the View Toolbar, making it accessible at all times. The other icons displayed in order of left to right are as follows
Snapping Toggle Options
Snap to geometry | |
Smart Snapping | |
Snap to Grid |
View Controls
Toggle Pan / Twiddle View | |
Zoom to box | |
Zoom to drawing | |
Zoom to selection |
Toolpath Drawing Toggle
Toggle 2D Toolpath Drawing | |
Toggle solid 2D Toolpath Drawing |
3D Drawing
Toggle drawing of material block |
Tile 2D & 3D View Windows
Stack 2D and 3D View windows vertically | |
Stack 2D and 3D View windows horizontally |
Two-Sided Machining
When you are working on a two-sided job additional icons will appear on the View Toolbar. On the left you will see an icon indicating whether the job you are working on will be flipped horizontally or vertically. This is important because the software will automatically mirror your toolpaths and geometry around different axes depending on this setting. To maintain the correct alignment of your toolpaths you must physically turn the material on your CNC machine in the same direction as you have specified during the design process.
Turn horizontally from left to right | |
Turn vertically, end over end |
Note
This icon is just for you information and does not perform any operation; it is not clickable.
The next button indicates which side you are currently working on. It is a toggle button that can be clicked. Clicking this button swaps the active side of your job.
Top side is active, all operations will apply to the Top side. | |
Bottom side is active, all operations will apply to the Bottom side. |
Note
The rulers that border the 2D View are colored to provide a handy visual indicator as to which side is currently active. An Orange background indicates that the Bottom side is currently active and any drawing or toolpaths are associated with the Bottom Side of your design.
The final additional tool for two-sided job is on the right hand side of the View Toolbar and it allows you to toggle the 3D composite relief to show either the currently active side or your model only, or both sides of your model as a single solid block.
Toggle Two-Sided View |
Rotary Machining
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.
Toggle Wrapped 3D view. |
Vector Boundary
The Vector Boundary form allows you to create boundaries around selected vectors.
Offset Boundary
When this is checked ✓ the created boundary is offset outwards by the distance specified.
Rubber Band Boundary
When this is checked ✓ the created boundary is the result of stretching a rubber band around the currently selected vectors.
The images below demonstrate the difference between the two types of boundary that the form creates. The picture on the left illustrates the standard offset output and the one on the right shows the result when Rubber band boundary option is checked ✓.
Migrating Post-Processor POST_BASE
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.
Default Post-Processors
If you have not made any changes to your post-processor, you could find it again in the Vectric shipped database in the Post-Processor Management dialog and simply click 'Customise' to add it again to your My_PostP folder.
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.
The base does not need to change
In this guide, we will go through how to replace the POST_BASE statement. We will never have to alter the base post-processor (referenced in that statement), but only the post-processor containing that statement. Please always back up your file first.
Check your output
Save some toolpaths using this new post and check the output!
What is a Base Post
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.
Summary of Migration
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.
Step-by-Step Example
Again, assuming the Next Wave post-processors
Next_Wave_CNC.pp
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]"
Next_Wave_CNC_mm.pp
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]"
Changes Summary
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,
POST_NAME
UNITS
LASER_SUPPORT
- Various variables
- The
HEADER
section
We have to ensure that those things are kept the same in the new Next_Wave_CNC_mm.pp
.
Steps
This will serve as a rough set of steps on how to approach this.
- 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.
- Go through the old inheriting post-processor (Next_Wave_CNC_mm.pp) and copy / replace the variables and sections.
- 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.
Check the result
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
.
Check your output
Save some toolpaths using this new post and check the output!
Toolpath Tree
The Toolpath Tree is located at the bottom of the Toolpath Tab below the Operations section (toggle tab visibility using Shortcut key F12).
This area displays in a tree , the name of each calculated toolpath with a check-box to turn the visibility of the toolpath in the 3D View on and off. The icon next to the check-box shows the type of tool selected for that particular toolpath.
Double-Clicking the name of any of the toolpaths will open up the toolpath strategy window for that toolpath and allow edits to be made to it.
Right-Clicking on the toolpath shows a menu which is described in more detail in the Right Click Menus Page.
Sheets Filter
The Sheets Filter, located just above the toolpath tree itself, allows you to filter the toolpaths by sheet.
- Selecting a particular sheet from this drop down list will make that sheet active and the tree will only show the toolpaths associated with that sheet.
- If you select All Sheets from the drop down list the tree will display all toolpaths on all sheets. In this view, those toolpaths associated with inactive sheets will be displayed faded out, although all operations can still be performed on them.
Toolpath Groups & Sheets
Toolpath groups are not associated with any sheet and so will be shown in all circumstances.
Up and Down Arrows
The up and down arrow buttons to the right of the window allow the user to move the selected toolpath up and down in the list.
This will affect the order the Toolpaths are previewed in and if multiple toolpaths are saved as a single file, then this will be the order that the machine cuts them in.
Resizing
You can adjust the space available for the Toolpath list by clicking and dragging the divider that separates the Toolpath List from the Toolpath Operations section, up or down.
Two-Sided Job
The toolpath list shows the list of toolpaths on the current side only. The label at the top will change to indicate whether you're viewing the Top / Bottom sides. To view the toolpaths on the opposite side, just switch sides from the View Toolbar.
Toolpath Groups
It is possible to add groups into the toolpath tree to help with toolpath organization.
Adding a group
There are two ways to add a Toolpath Group:
- Right click on an empty space in the toolpath tree and click
- Or, right click and choose . This will take of the visible toolpaths and group them together.
Remove a Group
You can delete a toolpath group as you usually would delete any toolpath. Either via the right-click menu, or with the delete key. However when you delete a toolpath group then you will be asked if you want to keep the sub toolpaths or also have them deleted.
Add Toolpaths to a Group
You can move toolpaths in and out of groups by dragging them in the toolpath tree.
Model
Menu
| Create Component ► |
| Create Component From... ► |
| |
| |
|
Fluting Toolpath
Fluting Toolpaths machine along vectors while varying the depth of the tool, creating extremely efficient machined decorative patterns.
This toolpath is similar to the option to Profile On a selected vector. The difference is the toolpath at the end of each vector can be ramped to taper the cut. This can be used for cutting standard woodworking Flutes or can be used for artistic engraving and marking effects with other types of artwork. In this section the options on the form will be covered along with some examples of the use for different applications.
Selecting Vectors
When the Fluting Toolpath form is open, the selected vectors will have their start points indicated in the 2D View by solid square green nodes, this is important as it will determine which end the ramps are added depending on what options are chosen on the form. An image of this is shown below where all the start points are to the left end of the selected vectors.
If you need to move the start points, go into node editing mode (press N on the keyboard or select the node editing icon in the Edit Vectors section on the left tab).
Select the vector you want to change the start point Move the cursor over the end you want to be the new start point Press P on the keyboard or Right Click and select Make Start Point from the pop-up menu. Exit node edit mode (press N again) Reselect all the vectors you want to flute
Cutting Depths
Start Depth (D)
This specifies the depth at which the Fluting toolpath is calculated. When cutting directly into the surface of a job the Start Depth will usually be 0. If machining into the bottom of an existing pocket or stepped region, the depth of the pocket/step that you are starting from must be entered.
Flute Depth
This is the depth of the Fluting toolpath relative to the Start Depth; the total depth will be the combination of the Start and Flute Depth.
Tool
Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.
Flute Type
Ramp over complete length
Checking ✓ this option means the tool will ramp over the whole length of the toolpath. At the start of the selected vector/s it will be at the Start Depth and at the end of the selected vector/s it will have cut down to the Fluting Depth.
Ramp at Start
Checking ✓ this option means the tool will ramp down only at the start of the vectors to the Fluting Depth. The distance of this ramp can be specified using the Ramp Length or Ramp % options.
Ramp at Start and End
Checking ✓ this option means the tool will ramp down at the start of the vectors then will ramp up again at the end of the vectors. The distance of these ramps can be specified using the Ramp Length or Ramp % options.
Ramp Length
Checking ✓ this option means that the length of the ramp can be set to an exact distance entered into the box. The ramp distance is measured from the start and the end of the vector/s depending what Flute Type you have selected. If the distance entered is greater than the possible length of the ramp then the maximum length will be used, this would be the same as choosing Ramp over complete length. When you choose Ramp at Start it is possible to specify a ramp length which is up to the length of the vector/s. When Ramp at Start and End is checked, ✓ the maximum length possible would be half way along the vector/s as after that it would start to ramp up again.
Ramp %
Checking ✓ this option means that the length of the ramp can be specified as a percentage of the maximum possible ramp length (controlled by the length of the selected vector/s and chosen Flute Type). When you use this with Ramp at Start selected then 100% would be the whole length of the selected vector/s, the ramp length would be a percentage of this distance for each one. When you use this with Ramp at Start and End then 100% would be the half length of any of the selected vector/s. The ramp length would be a percentage of this half-length. In this situation using a 50% value would give you a Ramp from the start which was ¼ of the vector length and a ramp from the end which was also ¼ of the vector length.
Ramp Type
Linear
Selecting the Linear type will create a ramp which is a diagonal line (following the vector) from the Start Depth to the Flute Depth. Below you can see a Linear Ramp Type shown from the side. This ramp is set to only ramp from the start and to go 50% of the flute length.
Smooth
Selecting the Smooth type will create a curved ramp (following the vector) from the Start Depth to the Flute Depth; this will smoothly transition from the ramp into the full depth of cut. You can see an example of this shown in the image below.
Fit Curves To Vectors
This function allows the user to fit arc, Bezier curves or straight lines to selected vectors. The newly created vectors will be approximated based on a user defined tolerance. Using this function can aid with smoothness for some toolpath options and also help to simplify data for modeling purposes.
Fitting Type
Circular Arcs
Checking ✓ this option means the selected vectors will be approximated using arcs:
Bezier Curves
Checking ✓ this option means the selected vectors will be approximated using Bezier curves.
Straight Lines
Checking ✓ this option means the selected vectors will be approximated using straight lines.
Tolerance
The value which is set in the Tolerance area determines how closely the original vectors will be approximated. The newly created, Arcs, Beziers or Lines will be generated within a distance of the original vector which is plus or minus the specified Tolerance value. The smaller the value the closer to the original the new data will be but it will also mean more data points will be used. A larger Tolerance will not be as accurate to the original but will have less data points.
Keep Sharp Corners
Checking ✓ this option will make the Curve Fitting routine keep sharp corners which have a difference greater than the Max Angle value specified. Any corners where the difference in angle is less than this value will be modified within the specified tolerance.
Replace selected vectors
Checking ✓ this option will delete the current vectors and replace them with the new curve fitted vectors. Un-checking it will keep the original vectors as is and in addition create new curve fitted vectors. The new vectors will always be created on the currently selected Layer.
General Workflow
VCarve Desktop has been developed to allow the production of decorative and artistic dimensional carved parts. As well as drawing and modeling tools, it includes both 2D and 3D machining, along with 3D V-Carving / 3D Engraving to allow a huge variety of jobs to be produced as quickly and easily as possible.
Workflow Logic
- Layout 2D Design:
- Import Vectors
- Draw Vectors
- Import Bitmaps
- Create 3D Components:
- Create shapes from 2D design vectors
- Create (texture) shapes driectly from bitmaps
- Import 3D Clipart and models from other CAD systems
- Manipulate 3D components to create the 3D composite model using the component tree:
- Change location, depth, size, angle etc.
- Group and change relationship to other components
- Create 2D, 2.5D or 3D toolpath:
- Create or edit vector boundaries for toolpaths
- Specify tool details for each strategy
- Preview Final Part:
- Visualize the part as it will actually look.
- Create proof images for customer.
- Check estimate for cutting time
- Save the CNC Code: Save the final cut file to send to the CNC machine
Design
VCarve Desktop includes drawing and editing tools that allow designs to be created and modified. Functions for vector creation and editing are very easy to use and multiple design elements can also be drawn or imported, scaled, positioned and interactively edited to make a new design. Text can also be created using any TrueType or OpenType fonts installed on your computer, or the single stroke engraving fonts supplied with the software.
Model
Existing 3D models can be imported to be incorporated into a design, these could be 3D Clipart that has been purchased and downloaded or models from other CAD design systems in a supported format.
Toolpath
A comprehensive set of 2D, V-Carving, Engraving and 3D toolpath strategies provide you with efficient ways to use your tooling to carve the finished part. This process is usually relatively independent of drawing or modeling (although toolpaths are often created directly from some artwork or 3D composite models). VCarve Desktop provides simple interface buttons to toggle screen layout to assist the shift in focus from design to toolpathing.
Output
Finally you can use VCarve Desktop's large selection of post-processors to save toolpaths in precisely the format that your particular CNC machine tool requires.
Signing In
Signing into the software gives users more benefits when it comes to your tool database backups and licence updates.
How to Sign In
You can sign in using different methods,
- Through the Licence Dialog as a more convenient method for entering your licence details.
- Through the button at the top right bar.
- In the Tool Database dialog to be able to back up and retrieve your database.
- In the Clipart Tab to be able to access your free clipart more conveniently.
Vector Texture
Repeating texture patterns can be created using the Create Vector Texture tool. These vectors can be machined in a variety of ways to create attractive textures.
To use the tool click the icon on the drawing tab. If required, select any contours that you wish the pattern to be created within. By using the sliders and edit boxes on the form the style of the created pattern can be varied. Click Preview to see a preview your created texture as you adjust the form's parameters. When you are happy with the preview, click OK to create the pattern.
Angle
The lines in the texture are created at an angle. This value can be set to any value between -90 degrees and 90 degree.
Line Spacing
The line spacing controls the distance between the contours created by the tool. Use the edit box labeled Max. Spacing to enter a maximum value of line spacing. The slider underneath the edit box controls the degree of variation in the line spacing. If the slider is to the far left then this mean variation is at a minimum and so the lines are evenly spaced. If the slider is to the far right the variation is highest and so the distance between created contours varies between zero and the maximum spacing specified.
Wave Parameters
Within this section of the form the created pattern can be made to behave in a wave-like fashion. This wave is controlled by two parameters: the amplitude and wavelength.
Wavelength
The wavelength describes the length over which the contours shape repeats itself. A bigger wavelength gives a long wave while a small wavelength gives a short wave.
Amplitude
The amplitude describes the height of the wave. Larger amplitude means a taller wave and smaller amplitude means a shallow wave.
Noise
The noise slider controls the degree of randomness applied to the above values and can be used to create less regular patterns.
Vector Layer
To create the vectors on a new layer make sure the check box labeled Place Vectors on Layer is checked ✓ and enter the layer name into the edit box labeled Name.
Job Setup Form
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited. It allows to create following types of job:
Job Setup - Rotary
The Job Setup form is displayed whenever a new job is being created, or when the size and position of an existing job is edited.
In most cases a new job represents the size of the material the job will be machined into or at least an area of a larger piece of material which will contain the part which is going to be cut. Clicking OK creates a new empty job, which is drawn as a gray rectangle in the 2D View. Dotted horizontal and vertical Grey lines are drawn in the 2D design window to show where the X0 and Y0 point is positioned.
Job Size
Length
Length of the material
Diameter
Diameter of the material
Units
Whether the job units are measured in mm or inches
Z Zero Position
Indicates whether the tip of the tool is set off the rotation axis (as shown in the diagram) or off the surface of material for Z = 0.0. For the best accuracy using Cylinder Axis option is recommended
XY Datum Position
This datum can be set at any corner, or the middle of the job. This represents the location, relative to your design, that will match the machine tool when it is positioned at X0, Y0. While this form is open, a red square is drawn in the 2d view to highlight the datum's position.
Use Offset
This option allows the datum position to be set to a value other than X0, Y0.
Orientation
This option selects along which axis the material block will rotate.
- Selecting Along X Axis means that X coordinates represent movement along the cylinder, whereas Y coordinates represent the angle around the cylinder.
- Selecting Along Y Axis means that Y coordinates represent movement along the cylinder, whereas X coordinates represent the angle around the cylinder.
Flip Design
When this option is enabled, the design will be flipped when the orientation is changed
Design Scaling
When editing the Job Size parameters of an existing job, this option determines whether any drawings you have already created will be scaled proportionally to match the new job dimensions. If you wish to preserve the existing size of your drawings, even after the job size has changed, leave this option unchecked. With this option checked, your drawings will be re-sized to remain in the same proportion and relative position within your new material extents when you click
Modeling Resolution
This sets the resolution/quality for the 3D model. When working with 3D models a lot of calculation and memory may be required for certain operations. Setting the Resolution allows you to choose the best balance of quality and speed for the part you are working on. The better the resolution quality chosen, the slower the computer will perform.
As this is completely dependent on the particular part you are working on and your computer hardware performance, it is difficult in a document like this to recommend what the setting should be. Generally speaking, the Standard (fastest) setting will be acceptable for the majority of parts that Aspire users make. If the part you are making is going to be relatively large (over 18 inches) but still has small details, you may want to choose a higher Resolution such as High (3 x slower) and for very large parts (over 48 inches) with small details then the Highest (7 x slower) setting may be appropriate.
The reason that the detail of your part needs to be taken into account is that if you were making a part with one large item in it (e.g. a fish) then the standard resolution would be OK but if it was a part with many detailed items in it (e.g. a school of fish) then the High or Highest setting would be better. As previously stated these are extremely general guidelines as on slower/older computers operations with the highest setting may take a long time to calculate.
As the Resolution is applied across your whole work area it is important to set the size of your part to just be big enough to contain the part you plan to carve. It would not be advisable to set your material to be the size of your machine - e.g. 96 x 48 if the part you plan to cut is only 12 x 12 as this would make the resolution in the 12 x 12 area very low.
Appearance
Clicking will pop up a dialog allowing you to set the color or material effect which will be applied to the base 3D model. It is possible to change this at any time and also to apply different colors and materials to different Components using the Component manager. See Preview Toolpaths to learn more about different material settings and adding custom material effects.
Import 3D Model into Single or Two Sided Job
Initial Orientation
Choose one of the 6 options to determine the most suitable direction on the model that defines the top surface (upper Z) that you want to use when it's converted into a Component.
You can also use the five options for Rotation about Z Axis to modify the position of the part being imported at this stage.
To rotate the model interactively, the dynamic handles in the 3D view can be used. The red, green and blue circles allow for rotation about the X, Y and Z axes respectively, while the central grey sphere can be used for rotating around all three axes simultaneously.
Model Size
Lock XYZ ratio
Un-checking this option allows the model to be distorted from its original shape. This means independent X, Y and Z sizes can be entered. Leaving it checked ✓ fixes the ratio so it cannot be distorted. Instead it will automatically scale the other axes as you enter new values for X, Y or Z.
Apply
Applies the values you have entered for the X, Y or Z dimensions.
Many mesh files do not inherently have the units that they were made in embedde in the files, so the software is not able to tell if the files are supposed to be inches or metric, they will just have a particular value. Therefore it is quite common to need to scale the part from inch to metric or vice versa. If you import your model and you wish to work in inches and the file seems very large or if you work in Metric and the file seems very small then you will probably need to use the Scale mm/inches option. The next two items on the form cover this need.
Units
Choose the unit of measurement (mm or inches) that you are working in, within the part the file is being imported into.
Changing the units will result in resizing the model. For example, if you had 5x5 mm dimensions, they would become 5x5 inches so the model becomes a lot larger.
Scale mm/inches
Scales the X, Y and Z values up or down depending which Unit option is selected. If mm is selected then the software assumes you want to scale the values up so multiplies the current values by 25.4, if inches is selected it assumes you want to scale the values down and divided them by 25.4.
Center Model
The button which will move the center of the model's bounding box to datum position (XYZ zero). This is particularly useful if you intend to unwrap a model for rotary machining. This may change the Zero Plane position in the model.
Apply Perspective along Z
Checking ✓ this will enable you to apply a perspective distortion to the model along the Z axis by using the slider. Points on the model closest to the observer will become further apart as the distortion strength is increased - this makes the model appear as if it is coming out of the screen.
Position & Import
Selecting this button will take you to the Position & Import dialog
Cancel
Cancels the Import function and returns to the standard Modeling Tab icons.
Texture Toolpath
The 3D Texture Machining functionality uses a specialized toolpath algorithm and the shape of the tool to generate a textured finish on the part.
Tool
Clicking the button opens the Tool Database from which the required tool can be selected. See the section on the Tool Database for more information on this. Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database. Hovering the mouse cursor over the tool name will display a tool tip indicating where in the Tool Database the tool was selected from.
Texture Settings
Use selected vectors as pattern
By default this option is unchecked and the texture form will generate a random texture pattern using any selected vectors as a clipping area. If this option is checked, ✓ the currently selected vectors will be used as the pattern for the texture and the only options available will be 'max. Cut Depth' and 'min. Depth' to control the depth of the cuts along the selected vectors.
Ramp at start and end
This option is only available when using selected vectors as patterns. If this option is checked ✓ each of the selected contours is cut using a fluting move, otherwise each of the contours is cut with a regular profile move. The resulting textures may look very different because of this small change.
Max. Cut Depth
The maximum depth any of the carved scallops will be machined to and is specified in the job units.
Min. Depth
Using the slider this is specified as a percentage (%) of the Max. Cut Depth and controls the minimum depth any of the scallops will be machined to.
Note
For example, with a Max Cut Depth = 0.200 inches and a Min Cut Depth of 0.050 inches, the depth of the carved scallops will range randomly between 0.200 inches and 0.050 inches.
Max. Cut Length
Specifies the maximum length for any of the carved grooves and is specified in the job units.
Min Length
Using the Slider this is specified as a percentage of the Max Cut Length and controls the minimum length any of the carved grooves.
Max. Overlap %
The percentage (%) of the Max Cut Length that each scallop is allowed to overlap the adjacent scallop running along the cutting direction. Where, 1% will result in almost zero overlap of adjacent scallops 50% will result in some of the scallops being machined half way over the adjacent scallop.
Variation
Using the slider this is specified as a percentage of the Max Overlap. Overlap variation of 100% = the Max Overlap and random pattern Overlap variation of 1% = No Overlap and an almost constant pattern.
Stepover
The distance between each parallel set of lines of carved scallops.
Angle
The direction the texture is machined across the surface, an angle of zero is parallel to the X axis, examples of setting the angle to 45 and 90° can be seen below.
Boundary Vector Offset
If you enter a value in this field, the texturing will be offset from the boundary by the specified amount. If you are texturing in a recess, you should enter a value here up to the radius of the tool to avoid the walls of the recess being damaged by the tool.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Project toolpath onto 3D Model
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.
Note:
When a toolpath is projected onto the 3D model, its depth is limited so that it does not exceed the bottom of the material.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Edit Sheet Form
The Edit Sheet form is displayed when editing one or more sheets on the Sheet Management Tab. The form is slightly different depending on the job type:
Create Zero Plane
Creates a component that is the size of your job setup with a height of Zero.
3D Finish Toolpath
Finish Machining is used to machine the final pass on the finished 3D part.
For most 3D Finishing cuts a Ball Nosed end mill is used with a reasonably small stepover (8 - 12% of the tool diameter is typical). Variations on this tool type such as a tapered Ball Nosed cutter will also work and may offer more strength with smaller tool sizes. The size of tool will depend on the size of the part and the detail within the 3D part. Use the preview function to check the finish quality and detail; if they are not to a high enough standard then the job may require smaller tooling or a smaller stepover. 3D cutting is always a tradeoff between time and quality and an optimum balance of tool size, finish quality, and time to cut. The choices made will always depend on an individual's personal preferences or the specifications of the job.
Note
The finishing toolpath is always a single pass, and it does not use the tool's pass depth. Please ensure that your Roughing Toolpath's Machining Allowance is set appropriately for the tool used in Finishing to avoid damaging the bit.
Tool Selection
You can select any number of tools you wish to use to create this toolpath. When multiple tools are chosen then the first tool removes as much material as it can, all subsequent tools in the list will remove as much material as it can from any previously unmachined areas. If multiple tools are selected then the order of the tools in the list should match the order they will run on the machine.
Note
Sometimes an allowance will be left on for the final tool to remove.
Clicking the button opens the Tool Database from which the required clearance tool can be selected and added to the list.
Clicking the button will remove the selected tool from the list.
Clicking the button opens the Edit Tool form which allows the cutting parameters for the selected tool to be modified, without changing the master information in the database.
Clicking the up and down arrow buttons will move the selected tool up and down the list respectively.
Machining Limit Boundary
The machining limit boundary is the area in which the tool will operate. There are several options:
Model Boundary The combined boundaries of all the components in this job are used. This is the area of the composite model which has components on it. Note: this is not the boundary of the selected models.
Material Boundary The boundary of the entire material block is used.
Selected Vector(s) Selected vectors are used as the machining boundary.
Selected Level The combined boundaries of all the components on the specified level. This is similar to Model Boundary, but only specific to the named level.
Boundary Offset
If you are machining a raised object, often the tool will not fully machine down the edge. This field is used to specify an offset to the selected machining boundary to increase its size to allow the tool to go past the actual edge if needed.
Area Machining Strategy
There are two choices of the type of fill pattern that will be used to machine the area with the toolpath; Offset and Raster.
Offset
Your choice of Climb or Conventional cutting will largely be dictated by the material that is being machined and you're tooling options. Talk to your tooling suppliers for details about what is most appropriate for your specific application.
Raster
Calculates a raster pattern (lace cut) projected onto the 3D surface and machined inside the selected vector(s), with control over Raster Angle - Between 0 and 90°. 0° will give you a pattern that is mainly parallel to the X axis and 90° is mainly parallel to the Y axis.
Stepover Retract
The Stepover Retract Value can be applied to the Offset Machine Strategy. If the value you enter is greater than 0 then the tool will lift off the surface of the composite model by this amount when stepping between each offset contour. Depending on your material and tooling, adding a small lift will eliminate perpendicular tool marks between the toolpath contours to potentially improve the finished surface.
Note:
If the Stepover Retract Value specified is not large enough to allow the machine to lift the tool over the previous cusp height then you will receive a warning. This warning is simply informing you that with a Stepover Retract value of this size then you will not eliminate perpendicular tool marks.
Rest Machining
Rest machining is a technique which uses multiple tools to try and optimize for machining time, material removal and tool lifetime. A series of tools can be chosen, with each tool removing any remaining material that the previous tool was unable to machine. If multiple tools are selected then rest machining will be used.
Minimum Detail
The minimum detail value and corresponding slider controls how small an unmachined area should be if it is going to be ignored by this particular tool in the toolpath. The result of finish maching with one tool will always leave areas of the model that are not completely machined. Often these unmachined areas are so small that it is not desirable to have a smaller tool to try and machine them. For example, it is unlikely that we would want to have the smaller tool try to remove the unmachined cusps of a previously cut toolpath.
Setting the minimum detail is likely to be a compromise between achieiving greater detail versus reducing machining time.
Boundary Offset
The boundary offset value specifies a value that every unmachined area will be offset by. A low value for the boundary offset will result in this tool machining lots of smaller areas. A high value will result in this tool machining fewer but larger areas.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Quick Engraving Toolpath
This form is used specifically for calculating engraving and marking toolpaths.
Depth / Pressure
When using Conventional Engraving and End Mill cutters the Depth to engrave / mark is specified and this z depth dimension is output in the toolpath file sent to the CNC machine. The 3D Preview of these toolpaths shows the specified depth of engraving.
When using a Diamond Drag marking Tool the Pressure setting is used to pre-load the spring to ensure the tip of the diamond stays in contact with the material surface, especially when marking uneven surfaces. The 3D Preview of the depth these toolpaths will mark using the Angle of the diamond and the Width of the Line.
For example, when using a 90° Diamond Drag Tool with a 0.010 inch Line Width specified. The depth shown in the 3D preview will be 0.005 inch (with 90° the depth = half the line width).
The ratio of Depth to Line Width will change when using diamond drag tools with different tip angles. When the option to use a Nose Cone is selected (see below) the actual depth specified on the form is used when previewing the toolpath in the 3D view.
Strategy
When using the Quick Engraving Form the Stepover for the cutter is specified on the form and is NOT automatically set from the Tool Database.
The selected text or vectors can be Outlined or Filled.
Outline
The tip of the cutter runs on the selected lines engraving / marking the material surface
Fill
A pattern is used to engrave / mark inside the selected text or vectors. There are 3 fill pattern options.
Use Nose Cone
A nose cone is often used when engraving or marking material that is not flat. The nose cone is spring loaded forcing it to slide on the surface of the material. The engraving cutter is set to extend / protrude out of the bottom of the nose cone by the depth of engraving / marking required. This is typically set at around 0.010 inches to 0.020 inches.
When the option to use a Nose Cone is selected the actual depth specified on this region of form is used when previewing the toolpath in the 3D view.
Number of Passes
This option runs the cutter multiple times divides over the toolpath pattern.
Immediate Output
Once calculated, your toolpath is stored in the central Toolpath Tree and can be saved, edited or output to your machine at anytime using the command. In addition though, this form also includes a convenient Immediate Output section that allows you to save or send the most recently calculated toolpath directly from this form without having to close it.
Post Processor
Use this drop-down list to select the post-processor for your machine.
Add side to toolpath name
If you are creating aligned toolpaths for a two-sided part, this option automatically adds the side name to the toolpath name as it is saved or exported to help keep your toolpaths organised.
Output direct to machine
If your post-processor supports direct access to your cnc machine (including machines supported by VTransfer), this option will be available. Selecting this option will bypass saving the toolpath to disk and instead send it straight to the direct output driver.
Trim Objects
The trim tool allows you to trim all the objects inside a given boundary. It is much more efficient than manually trimming all the contours with the trimming scissors, and allows the trimming of closed contours, open contours and components.
To use:
- Select objects you wish to be trimmed
- Select the object you wish to trim against (hold shift to add to selection)
- Choose to clear inside or outside
If the Clear outside boundary option is selected then all the objects that intersect this boundary are clipped, and the area outside is removed. If the Clear inside boundary option is selected, then the parts of the selected objects which lie inside the boundary are removed.
If you want to use multiple vectors for the trimming boundary, they must be grouped for trimming. To group a collection of vectors select the vectors, right click and choose Group Objects from the drop down menu, alternatively select all the vectors and press the G key.
Refit Curves After Clipping
In order to clip curves the trim tool will convert them to curves consisting of many small lines. If this option is selected then after clipping has happened the vectors will be converted to curves.
PDF Export
The PDF Export form allows vectors within your drawings to be exported into PDF format.
Vector(s)
Export All
Selecting this option will export all of the vectors contained on the specified sheets and layers.
Export Selected Only
Selecting this option will export only the vectors which are currently selected and on the specified sheets and layers.
Sheets
The sheets you wish to be exported to PDF can be selected from within this section. Clicking will deselect all of the sheets and clicking will cause all of the sheets to become selected. You can also manually select/deselect individual sheets by clicking on the check box to the left of the sheet name.
Note
Each sheet will be saved as a separate page within the PDF file.
Layers
The layers you wish to be exported to PDF can be selected from within this section. All the visible layers with content on them will show up in this list.
When All visible layers is chosen all of the vector layers will be selected. Only vectors on the layers selected will be exported into the PDF file. When Selected layers only is chosen individual layers can be manually selected/deselected by clicking on the check box to the left of the layer name.
Options
Export Job Bounds - If this option is selected a vector representing the boundary of the job will also be output to the PDF file.
Clicking will prompt you to choose a filename and location for your file and save your drawing in PDF format at that location.
Rotate
For precise control of the rotation, or to use a point other than the selection's center as the rotation center, you can open the rotation form from the Drawing Tab.
Selected items in the 2D View can be rotated to a new orientation using this tool. The rotation options form can be activated from the tool icon on the Drawing Tab. Alternatively you can use the interactive transform mode (where the form is not required) directly from the 2D View.
With this form open the additional Pivot Point handle is available (two concentric circles initially positioned at the center of your selection) for you to click and drag in the 2D View. The Pivot Point (around which the selection will be rotated) responds to the currently enabled snapping options to help you to position it precisely on significant locations within your artwork. Hold down the Shift key to temporarily disable snapping while you drag the Pivot Point.
Pivot Point
On the form there are also six radio button options for snapping the rotation Pivot Point to the selection itself or to a precise position. The first five options allow you to snap to the corners and center of your selection.
Use Coordinates
The X and Y edit boxes allows you to precisely specify the position of the Pivot Point. This is also the option that will be selected by default if you drag the pivot point using your mouse directly in the 2D View.
Type of Rotation and Angle
This controls what the angle value does.
- Relative will simply rotate the object by the given angle. For example, you can enter a small angle, and then rotate multiple times to nudge the object a little bit at a time. A positive angle results in a counter clockwise rotation. A negative angle results in a clockwise rotation.
- Absolute will set the rotation of the object to the given angle. For example, setting a zero angle here will reset the rotation of the object back to its original orientation (as long as the rotation hasn't been baked).
Keep in mind that when rotating an object, it's rotation is maintained so that you can restore the rotation or scale along its original axes later on if required.
Interactive Rotation
Generally the most convenient way to rotate an object in the 2D View is to use interactive transform. This mode is initiated by clicking the selected object twice with the cursor. The process is:
- Select the object by clicking on it in the 2D View (or multiply select objects using box selection or by shift-clicking on them).
- Click the selection a second time to activate the interactive options rotation handles on the selection box.
- Click and drag on the blue handles (solid squares) at the far corners of the selection to rotate it.
Note
Holding down an Alt key when dragging to rotate the object snaps to angular rotation steps of 15° increments.
Open a File
This option opens the File Open dialog window, allowing Aspire files (CRV) and importable 2D vector files to be selected and opened.
Laser Cut And Fill
Note
The Laser Module is available as a paid-for add-on to the software. The features are not included in your software by default. To find out more about the Laser Module, please go to https://vectric.com/laser-module
Laser Cut - Fill is used for cutting out shapes or marking areas.
Cut-outs can take into account the kerf, or width, of the laser beam to maintain the precise internal or external size the selected vector shapes. Shapes can also be filled with stripes or hatching to create simple shading effects.
Tool Selection
Select Tool
This button opens your database of previously stored laser settings for different jobs and materials. When a setting is selected fromt the database it will be used to populate the key fields in this section. You can subsequenlty modify these values when calculating the laser toolpath. Modifying the settings on this form will not alter the original stored settings within your database.
Power
This value sets the proportion of the maximum laser power from your machines that will be used for this tool path.
Move Speed
This specifies the maximum speed that your machine will move during cutting or engraving moves. The units are determined by the database setting that was originally selected.
No. Passes
The machine can repeat a tool path several times to cut through thicker material. This value sets the maximum depth the machine will attempt to cut with each pass to achieve the final Cut Depth.
Overscan
Overscan allows the user to have the laser pass beyond the edge of the lasered area, to account for deceleration of the machine which would otherwise result in a darker edge to the laser burn. Overscan is machine dependant and the user will need to run some test images to identify how much overscan to use on their machine at a given feedrate to eliminate overburn at the edges of the lasered area.
Strategy
Based on the selected vector shapes in your drawing, this toolpath offers four distinct strategies.
Cut Outside / Right
Selecting this option will run the laser around the outside of your selected vector shapes (or along their right-hand edge, if they are open vectors). The actual path of the laser is automatically offset from the orginal shape according to the kerf width of the laser. As a result, the external dimensions of the resulting physical part precisely match the size of the original vector drawing. This strategy should be used for cutting out shapes to precisely the correct dimensions.
Cut Inside / Left
This option will run the laser around the inside (or left-hand edge) of your selected vector shapes, allowing for the kerf of the laser. This strategy is typically used for cutting holes, slots or sockets where the remaining recess has precisely the same dimensions as the original selected vector drawing.
Cut On
This option will run the center of the laser beam along the selected vector. No offsetting or kerf compensation is required.
Hatch Fill
This is a marking or 'shading' strategy which profiles along the selected vectors and then fills-in the shapes with stripes. When this option is selected the additional Stepover, Hatch Angle and Cross Hatch options will also become enabled - see below for more information on these.
Allowance
This setting allows you to add an additional offset for the Cut Outside, Cut Inside strategies without adjusting the laser kerf settings and can be useful for easing or tightening the fit of shapes resulting from these cuts.
Note
This option is not applicable to the Cut On or Hatch Fill strategies and will be disabled if they are selected.
Stepover
When creating hatch fills, this option determines the spacing between the hatch lines. It is only available when the Hatch Fill strategy is selected.
Hatch Angle
When the Hatch Fill strategy is selected, this option determines the angle of the hatching lines used.
Fill Together / Fill Regionally
These options will change how areas separated by spaces are treated. In the example of the word "Test" with Fill Together selected the letters will be treated as one whole space to be filled whereas with Fill Regionally each letter will be treated separately as its own individual region.
Cross Hatch
Checking this option will create a cross hatch fill instead of a single set of lines.
Outline
Selecting this option will then create a defined outline around a chose vector. If unchecked there may be gaps around the edges if the stepover is large enough whereas when checked an outline passing around the outside will appear.
Position and Selection Properties
Safe Z
The height above the job at which it is safe to move the cutter at rapid / max feed rate. This dimension can be changed by opening the Material Setup form.
Home Position
Position from and to that the tool will travel before and after machining. This dimension can be changed by opening the Material Setup form.
Project toolpath onto 3D Model
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.
Note:
When a toolpath is projected onto the 3D model, its depth is limited so that it does not exceed the bottom of the material.
Vector Selection
This area of the toolpath page allows you to automatically select vectors to machine using the vector's properties or position. It is also the method by which you can create Toolpath Templates to re-use your toolpath settings on similar projects in the future. For more information, see the sections Vector Selector and Advanced Toolpath Templates.
Name
The name of the toolpath can be entered or the default name can be used.
Immediate Output
Once calculated, your toolpath is stored in the central Toolpath Tree and can be saved, edited or output to your machine at anytime using the command. In addition though, this form also includes a convenient Immediate Output section that allows you to save or send the most recently calculated toolpath directly from this form without having to close it.
Post Processor
Use this drop-down list to select the post-processor for your machine.
Add side to toolpath name
If you are creating aligned toolpaths for a two-sided part, this option automatically adds the side name to the toolpath name as it is saved or exported to help keep your toolpaths organised.
Output direct to machine
If your post-processor supports direct access to your cnc machine (including machines supported by VTransfer), this option will be available. Selecting this option will bypass saving the toolpath to disk and instead send it straight to the direct output driver.
Draw Circle
Circles can be created interactively with the cursor and Quick Keys or by entering the exact coordinates and diameter / radius with typed input.
Note
Pressing the Space-bar re-opens the last vector creation form you used. This is very useful when using other forms in between each shape you create.
Interactive
Cursor
The default mode and the procedure for drawing circle is:
Click and drag the Left mouse to indicate the center point followed by releasing the button at the required radius / diameter (depends on what is set on the form).
Note
Holding Alt and dragging creates a circle from the middlepoint.
As the cursor is dragged across the screen the radius is dynamically updated. The increments will depend upon your snap radius and the job size.
Quick Keys
The radius or diameter can be specified while dragging out a circle:
Type the value while dragging followed, by D if it's a diameter, or R if it's a radius:
Example:
1 2 R Gives a radius of 12
Exact Size
Circles can also be drawn by entering the required XY origin, selecting either Radius or Diameter and entering the required size on the form.
Click Create to update the circle.
Edit
Open the Draw Circle form and select the circle to modify.
The selected circle is displayed as a dotted magenta line. Edit the Center Point and Radius or Diameter
Click to update the circle
To modify another circle without closing the form hold a Shift key down and select the next circle.
Close the form
To finish drawing with the tool, you can :
Click Close on the form
- Press the key Esc
- Click the Right mouse button in the 2D View
Freehand Drawing
This tool will allow the user to draw both open and closed vector paths in a freehand style which closely mimics the flow of drawing with a physical pencil and really excels at creating quick initial design sketches and organic flourishes.
Optionally paired with a Windows compatible graphics tablet, this tool will enable you to draw your paths with a stylus, giving a more faithful simulated drawing experience.
The resulting image you see on screen still exists as vector information including automatically placed nodes and handles, meaning that you then have the option to use the same shape editing tools as any other path within the software to further edit and manipulate the vectors you have initially created with the Freehand Draw Tool.
Open paths with Freehand Drawing Tool
1. Under the create Vectors section of the Drawing panel > Select the Freehand Drawing Icon.
2. Left click and hold within the workspace to place a first point and the path will then follow the direction of your cursor. Whilst active the cursor will change to a Cross-hair and the drawn path will follow it's centre point.
Note
If Stabilisation is applied, a reticle will appear next to the cursor. This is explained under Freehand Draw Options below.
3. Release to place end point and finalise path.
Close Current Stroke
Whilst actively drawing an open path click TAB To join the the current point with the Path's start point creating a closed vector shape
Extend Existing open Vector path
In order to extend an existing open vector using the Freehand Drawing tool;
1. Hover your cursor over the point you wish to join from
2. Holding down Ctrl > within the immediate area of this point > Drag to draw path
3. Release to complete path.
Join On to Existing Vector
Whilst you are actively drawing a path with the held down, and you would like to join this to an existing open vector;
1. Press and hold Ctrl > Hover cursor over the Start or end point of another open vector
2. Release To complete path and join this to existing open vector line, creating one continuous path.
Freehand Draw Options
Smoothness
This option, controlled by the below slider, controls to what extent smoothing is applied when the is released and the path completed.
The further the slider is to the left the smaller the amount smoothing that is applied and any angular changes in direction will be retained once the is released and the path completed.
The further the slider is to the right the greater the level of the smoothing effect that is applied; Sharp angles are smoothed into curves and the path is simplified with fewer individual nodes created.
Stabilise
The stabilisation setting controls how much small movements with the mouse or stylus will be damped out whilst drawing.
This is controlled within the form by the below slider;
The further the slider is to the left, the less stabilisation is applied when drawing and even small changes in direction from the mouse/stylus will show in the resulting path.
The further the slider is to the right, the more stabilisation is applied and the tool will damp out small jitters in the mouse/stylus movement to produce a smoother path.
When an amount of stabilisation is applied a circle will be shown around the start point of the path when you start drawing and follow the end point of the path. Within the zone of this circle movement of the cursor will not extend the path. The cursor needs to move to the edge of this zone at which point the path will start moving towards the cursor. As cursor movements within this zone do not affect the path it also allows precise sharp changes of direction as you can move the cursor back into this deadzone then off in a different direction easily.
End Vector at Cursor
With this option unchecked; when the left mouse button is released, the end point of the actively drawn path will be placed in the centre of the reticle which appears to indicate the level of stabilisation being applied.
If instead you wish for the end point to be placed in the position of the cross hair cursor when the button is released, you can check the box next to this option. As the end point will remain the same regardless of the level of stabilisation applied, this can lead to greater accuracy in predicting the end of your drawn path.
Fade selected Bitmap
One of the many useful applications for the Freehand draw tool is for greater control over the tracing of imported bitmap images. By using the Fade selected Bitmap slider, the user can control the level of transparency for the selected Bitmap you are tracing over.
The further the slider is to the left - The lower the transparency of the selected bitmap, until completely opaque.
The further the slider is to the right - The level of transparency increases, giving the drawn path higher contrast against the traced image and making it easier for the user to distinguish on the screen.
Exiting Freehand Draw Form
Once you have completed your drawing and wish to exit from the freehand draw form, either;
- Click the
- Or Press the 'Close' button at the bottom of the form in the drawing panel.
Create Fillets
Fillets or radiuses can be added interactively at points where any two spans on a contour meet.
Creating Fillets
To use the filleting tool we select the icon from the drawing tab. Choose a radius for the fillet and the type of fillet you would like to use.
When the mouse cursor is near a node that can be filletted, the mouse cursor changes to show a check-mark ✓:
Fillet Type
Normal Fillet
This creates a standard corner fillet based on the Radius defined, typically this would be used for design purposes and not for editing a slot for fitting purposes. Below left the image shows the vector before filleting the two inside radii, on the right is the filleted version
Dog-Bone Fillet
This creates a circular cut-out style of fillet, the circles will be placed so the upper right part of the circle touches the original sharp corner and are created with the Radius specified. This option should not be used if the slot width and the tool are similar in size. Below left is the vector showing the slot before filleting, on the right is the filleted version using the 'Dog-Bone' option.
T-Bone Fillet
This creates a circular cut-out style of fillet, the circles will be created with the Radius specified. This option should be used if the slot width and the tool are similar in size so the slot can grow out to the side to ensure there is space for them to fit. Below left is the vector showing the slot before filleting, on the right is the filleted version using the 'T-Bone' option.
The placement of the fillet is an interactive process; you can choose which side of the 'corner' the T-bone filet is placed. If you click on a 'corner' the fillet will be placed automatically on the longest side. By clicking to the side of the corner you want the fillet placed you can choose which side the fillet is placed on.
Removing Fillets
Fillets can be removed in the same way that we add fillets: move the cursor over the fillet that you wish to remove.
If this fillet can be removed then the cursor shows a cross to indicate that it is possible to remove a fillet:
Clicking removes the fillet:
When removing fillets the software does not store what kind of geometry the fillet was created from. It always defaults to using straight lines to return the fillet to a sharp corner. As such if the fillet is across multiple spans or is derived from arcs or Bezier curves then it will not go back to its original state and instead it will remove the radius and extend two straight lines to create the new corner.
Extend Vectors
This tool allows you to extend two vector lines to their common point of intersection.
With the Extend Vectors tool active, moving the mouse pointer over the ends of open vector shapes (without clicking) will highlight a dashed preview extension line from that shape. The line will change dynamically as you move the mouse over the end spans of different open shapes. Clicking with the left mouse button at this point will set it as the target line to extend and the magenta line will remain visible.
The mouse can now be moved over existing spans along the length of the preview extension line, or over the end of another shape to create a second, intersecting, preview extension line.
Clicking on any of the intersection points indicated by the mouse cursor will extend the initial shape to that point and complete the operation.
The tool can be closed at any time using the button on the form. Right-clicking in the 2D View will reset the tool so that it is ready to select another target line to extend.
3D Toolpath Files
Files from Vectric's Cut3D, PhotoVCarve and Design and Make Machinist that include 3D toolpaths can be imported into VCarve Desktop using the main menu command: File ► Import ► PhotoVCarve, Machinist or Cut3D Toolpaths.
The 3D file must first be scaled to the required size before toolpaths are calculated, and then the complete file saved ready for importing into VCarve Desktop. These files can only be moved and positioned inside VCarve Desktop but cannot be scaled.
A Grayscale thumbnail of the 3D job is drawn in the 2D View with the X0 Y0 origin at the position it was set in Cut3D, PhotoVCarve or Design and Make Machinist. The associated toolpath(s) are also drawn in the 3D window and the names appear in the Toolpath list.
Positioning
To move the 3D design toolpaths open the 2D Window, click the Left mouse Twice on grayscale image (turns light Blue to indicate it's selected), then drag to the required position, or use the Move or Alignment tools for accurate positioning.
The toolpath(s) are automatically moved in the 3D window to the same XY position as the image.
Toolpaths for the example above have been calculated with the X0 Y0 in the middle of the 3D design. When imported into Cut2D the data is automatically positioned using the same coordinates, which places three quarters of the design off the job. In the second image the grayscale image has been moved to the middle of the job.
The 2D mirror and rotate drawing tools can also be used to edit the 3D data set.
3D toolpaths can also be copied using the Duplicate Toolpath command on the Toolpaths Tab making it very easy to use multiple elements from a single design on a job. The thumbnail preview is also copied for each toolpath, making it very easy to position additional copies of a 3D toolpath.
For example, a single design can be copied and mirrored to create Left and Right versions of a 3D design or to place multiple copies of a decorative design in the corners of a cabinet door panel as shown below.
Toolpaths for the 3D elements can be previewed along with the conventional Profile, Pocketing and Drilling toolpaths, and everything will be saved ready for machining.
A good example of where this functionality might be used in conjunction with PhotoVCarve is for making personalized picture frames that include the PhotoVCarve grooves plus descriptive engraved text and a decorative Profiled or Beveled border. As shown below:
Options
Imported toolpaths can also be edited to position them inside the material or to change the cutting parameters - speeds and feed rates can be changed.
Design and Make Machinist
When using a Design and Make Machinist file that includes multiple toolpaths, you must remember to edit the Start Depth for all of the imported 3D toolpaths.
Click the Edit toolpath icon or Double click on the toolpath name to open the edit form.
For example, after machining a half-inch deep pocket a PhotoVCarve design can then be edited to have a Start Depth = 0.5 inches and this will carve the photograph onto the base of the pocket surface.
Machine
Machine Configuration... | Opens Machine Configuration dialog. |
Add Machine... | Adds a new machine and opens Machine Configuration dialog. |
Install Offline Package... | Opens a File Dialog for selecting a package with Machine Configuration(s) |
Search for Machine Online... | Brings up Search for Machine Online dialog. |
Post-Processor Management... | Gives a list of all installed Post Processors and allow the user to Check the Changelog, Customise a duplicate of a Post Processor or simply View the Post Processors current formatting. |
Install Post-Processor... | Opens a File Open dialog box where you can install a post processor. |
Update Post-Processor Database | Downloads a latest version of the Post-Processor Database. |
Plate Production
This command is for designing and engraving multiple badges or nameplates using variables for positioning imported data from a text file list. The production plate functionality is typically used by engravers making badges from a database file supplied by a customer, but could also be useful for making nameplates for hotel rooms with consecutive numbering.
Procedure
Draw and Setup the Master Template
Create a New job and specify the Material Size to equal the Sheet size the badges will be cut from.
Layout the badge / plate at the required size and using the Text Tools add variables where imported data / text is required. Variables are defined using double exclamation marks ('!!') at the start and end of the variable name.
Calculate Toolpaths
Select and calculate the toolpaths for each of the elements on the design. For example, calculate an engraving toolpath for the text and logos and a separate Profile cut-out toolpath around the outer edge to cut out the design
Use the Plate Production Tool on the master template
With all of the vectors that make up the master template selected, click on the Plate production tool to open the Plate Production Dialog window.
The Plate Production Dialog
The left side of the Plate Production form is used to layout the plates / badges on the selected sheet of material, and shows the total number of plates that can be engraved / machined from each sheet of material.
Material Size
This is the material sheet size that the badges will be engraved onto. If the number and size of the badges requires additional sheets of material to be used the software automatically creates a separate layer for each sheet required.
Plate Size
This is the size of the selected Plate / Badge and is based on the bounding box of the selected vectors.
Sheet Margins
This specifies the border margin between the edge of the material sheet and the plates.
Independent margin spacing can be set for the Top, Bottom, Left and Right sides of the material
Equal Margins ensures the same space is added around all 4 sides of the plates.
Spacing
This is the horizontal and vertical spacing between each Plate / Badge.
Number of Plates
The number of plates that will fit on to the specified material sheet size is automatically calculated. This calculation takes the plate size and adds the Sheet Margins and Plate Spacing to determine the maximum number of plates that can be made from each sheet.
Toolpath Options
If toolpaths have been calculated for the master Template this option is available.
Checking ✓ this option automatically calculates toolpaths for all the plates / badges in the project.
Unchecking this option only creates the vectors for each plate / badge.
Import the Data to be Merged into the Template
The right-hand side of the Plate Production form is used to select the data that will be merged into the template, and how the data will be interpreted to create each plate / badge
Import the required text / data file using and select the appropriate format separator.
The data file is commonly created using a spread sheet such as Windows Excel. Use the option to Save As or Export to obtain the required file format that includes the correct Separator information.
Separator
The separator is the method used in the data file for dividing each set of information into columns. The most commonly used options are: Comma, Tab, Semicolon or a Space
First row is column names
It's very common for the first row of data in a file to simply show what each of the field names are, and this information is not used on the badge or plate. Checking the box First row is column names tells the software to start working with data from row 2
Assign the Variables to the data in the text file
All of the variables specified on the template - text with double exclamation marks '!!' on either side '!!' are automatically listed on the form. These variable names are each assigned to a data field (column of text) inside the data file.
Variable Assignment
Click to select a Variable Name then select the data field from the imported file that is required on each badge / plate i.e. the person's name
Repeat for each of the Variable Names listed on the form
Number Formatting
Variables can be assigned to Text from a data file - Names, Dept., etc. or to a Counter number that can be formatted and incremented using the Number Format options.
Calculate
Click to create all Badges and associated Toolpaths
If toolpaths have previously been calculated for the vectors in the Master Template, the option to automatically Create Toolpaths for each badge / plate is switched on in the bottom left corner of the form.
Close
Click to finish plate production and close the form
Multiple Sheets
Multiple Layers are automatically created if multiple sheets of material are required to engrave all of the badge data from the imported text file. Layer named Sheet 1 is displayed in the 2D view showing the badges on this sheet.
Each of the Sheets is on a different layer and can be set visible or invisible using the Layer Manager.
Multiple Toolpaths
When Toolpaths are automatically calculated, a separate toolpath for each operation on each sheet of material is calculated and named using the convention 'S1 - Name', where the Name is the name of the toolpath previously calculated for the template.
Machine Configuration Management
This dialog is used to edit and manage the list of machines for use in the tool database. It is also used for associating post-processors with those machines for use in Toolpath Saving. It can be accessed through the Machines Menu, the Tool Database dialog, or the Toolpath Saving form.
Machine List
List the machines added to the database. Selecting a machine activates it. This allows it to be edited in this dialog. In the Tool Database dialog, it results in switching the cutting data of the tools to be the set defined for the active material / machine (if any).
Add Machine
Add a new machine to the database and makes it active ready for editing.
Install Offline Package
Allows you to install a machine package which was downloaded from your V&Co account. If you are online, it may be better and more convenient to use the Search Machine Online tool directly from within the software.
Machine packages are preconfigured machine configurations which come pre-associated with compatible post-processors and ready with an initial set of Feeds & Speeds for a set of tools. This can all be done manually through this dialog as well, or edited subsequently following the install.
Search Machine Online
This takes you to the Search Machine Online dialog to download a machine package from our online services.
Duplicate Machine
Duplicates the active machine and makes the new machine active ready for editing.
Copy Cutting Data
This could optionally duplicate all the cutting data associated with the original machine for all the tools so that there is a new set of cutting data for the new machine as well.
Delete Machine
Delete the active machine and activate the next one up in the list.
Deleting Cutting Data
This is a destructive process deleting all the cutting data associated with this machine across all the tools.
Name
Allows us to set the active machine's name (if any). Two machines cannot have the same name.
The remaining parameters are optional and can be left empty. They define various common properties of the machine which may help you to identify them and us to tailor the behaviour in future versions.
Associated Post-Processors
This allows you to manage the list of post-processors associated with this machine configuration.
Through this, you can Add or Remove a post-processor. Right-clicking on the post-processor gives you some of the options available in the Post-Processor Management dialog, or set it to a fixed version.
Adding & Removing a Post-Processor
This will allow you associate a post-processor to this machine configuration by selecting it from the list of available post-processors.
You can also remove this association using the 'Remove' button. This will not remove the post-processor from your machine, but will simply disassociate it from the current machine configuration.
Post-Processor Version
Clicking the version displayed in the second Version column will popup a list showing the available versions of this post-processor.
- Latest (Vn) where n is the latest version: Allows to keep using the latest version of the post-processor along with subsequent updates we may ship to it.
- Vn where n is a version: Allows you fix the version of the post-processor you're using to version n. Subsequent updates to this post-processor will not be used unless you specifically update to it.
Removing a Post-Processor Version
There may be occassions where a version is removed for your version of the software (or for a future version) for fixing of major issues or because of an incompatibility with that version of the software.
Right-Click Options
You will get many of the options available to you in the Post-Processor Management dialog.
A couple of notes,
- will display your currently selected version of the post-processor
- will set a post-processor to be selected as the default post-processor when using in Toolpath Saving.
Apply Changes
Apply changes by clicking or . Clicking will discard any changes made.
Dimensions
This tool allows you to add a variety of dimensioning annotations to your vector drawing.
Creating Dimensions
Unless otherwise noted below, dimensions are created by following these steps:
- Select the dimension type you wish to need: length; height; width; angle or the radius or diameter of an arc.
- In the 2D View, click with the left mouse button to set the points the dimension needs:
For an Angle Dimension, the first point is the centre-point. - Click where you need the arrow-tips to be.
- Click to set the location of the dimension-line.
- Click to set where the annotation text will appear.
Editing Existing Dimensions
To edit an existing dimension while the form is open, hold down aShiftkey while selecting it.
Dimension Types
The dimension tool supports a number of different dimension types.
Length Dimension
Use this to dimension a straight-line length in any orientation between two points.
The text preview box will snap to to the middle of the dimension line, unless a Shift key is held down while dragging.
Vertical / Horizontal Dimension
These two options also allow you to select any two points, but the resulting dimension will be locked to indicate a vertical or horizontal distance (respectively) between the two points.
The text preview box will snap to the middle of the dimension line, unless a Shift key is held down while dragging.
Angle Dimension
This option allows any arbitrary angle to be measured. The process is similar to creating a 3 point arc. First you must pick the center of an angle you wish to measure - typically a corner point. The next 2 points clicked will set the extents of the sweep you are measuring. The next Click will determine the dashed dimension line positioning and the final click will set the position of the text annotation.
- Angle Dimensions' arrow-heads will pop outside small angles if there is not room to draw them inside.
- Angles are extended with a dashed extension-line where required, allowing the dimension to be placed anywhere. The text snaps to the angle center and the leader-line angle snaps to horizontal, vertical or diagonal (disable snapping by holding down aShift key).
- Angle Dimensions use a separate Decimal Places value to the other dimensions (as you change dimension-type you may notice the Decimal Places value change).
- Angle dimensions can now have up to six decimal places.
Arc Dimension
With this option selected you will only be able to select arc spans with the first click of dimension tool (Bezier curve spans are not supported). The second click will set the position of the dimension annotation, which will show the radius (or diameter) of the selected arc span.
- To display the diameter of an arc dimension simply check ✓ the Show Diameter box.
- Arc Dimensions recognise when a circle has been selected and allow placement anywhere around the circle. Arcs will now be extended with a dashed extension-line where required, allowing the dimension to be placed anywhere. The text snaps to the arc/circle center and the leader-line angle snaps to horizontal, vertical or diagonal (disable snapping by holding down a Shift key).
Note
Circles or arcs that are polygonized (from an imported file or from the Curve fit vectors command using Straight lines) are not recognized and cannot be dimensioned with this tool
Font Selection and Settings
This section of the form allows the user to change the settings for the dimension annotation, such as the font to be used, the height of the text and how many decimal places are required. The Offset field determines the gap left between the dimension markers and the vectors that are being measured.
Use Custom Text
You can check ✓ Use Custom Text to insert your own custom text. The text is stored per dimension, so you change between calculated and custom text without losing a dimension's custom text. When the form is first opened it defaults to calculated text.
Place Dimensions on Layer
By default this option is checked ✓ and the dimensions will be placed on a mid-gray Dimensions Layer. You can edit the name of the layer in the Name edit field. If a layer of this name does not exist, it will be created automatically.
Note
Dimensions can be edited. Hold shift while selecting the dimension you wish to edit or use the Undo shortcut Ctrl+Z to undo previously created Dimensions while still in the Dimensioning tool.
Join/Close by Moving End Points
Join Moving End Points finds the closest end points on 2 selected, open vectors, calculates the mid-point between them and moves the end points to this position.
Tool Database - Name Format
This dialog allows the editing of the name template used for naming tools with that tool type. It can be accessed through the name icon on any of the tools on the Tool Database dialog, and it will affect that particular tool or all tools with the same type.
Format
This field allows entering the name format / template that will be used for this tool (or tools of this type, controlled by the checkboxes).
The template contains variables of the format {Variable Name}
which will be substituted by their real value for the tool.
- For example,
{Tool Type}
will be End Mill for an End Mill tool and Ball Nose for a Ball Nose tool. - We can optionally format those the values in certain ways using modifiers
{Variable Name|Modifier}
. In the above example,{Tool Type|U}
would result in END MILL or BALL NOSE.
The list of all available variables and modifiers is available at the bottom of the page. It can also be accessed by right-clicking the field and selecting the variable.
Variables could relate to the tool geometry, cutting data or even machine and material being used. The tool name will automatically update within the current context. For example,
- We have materials MDF and Oak and a tool with the name template
{Tool Type} {Diameter} {Material Name}
. The tool is an 0.5 inch End Mill. - When the MDF material is active, the name of the tool becomes End Mill 0.5 MDF. When it Oak is active, it becomes End Mill 0.5 Oak.
- When the tool is selected for toolpathing, the name of the tool with the correct material name will be used allowing you to see straight away which variant of the tool you've used.
Set as Default
This dialog can be used to manage name formating for each tool type. When a format is set as the default, any subsequently created tools will be named according to that format by default. Setting a format as a default (optionally) allows you to do just that.
Any tool which does not have the default name format for its type can be restored using the next to the format field.
Update existing tools
When changing the name format of a tool, there is the option to rename all the other tools with with the same Tool Type.
If you select this, you will have the option to either
- Rename all the tools that had a matching name.
- Rename all the tools indiscriminantly.
List of Variables
Here is the complete list of variables that can be used in the format.
In some cases, we may not be able to find a valid value. For example, if we use the {Material Name}
when no material is active. In this case, we will simply keep the name of the variable in the tool name. This should not happen if the tool is valid / suitable for toolpath selection.
Variable | Type |
---|---|
Geometry | |
| String |
| String |
| String |
| Float |
| Float |
| Float |
| Float |
| Float |
| Integer |
| Integer |
Cutting Parameters | |
| String |
| String |
| Float |
| Float |
| Float |
| Float |
| Integer |
| Float |
| Float |
Feeds & Speeds | |
| String |
| Float |
| Float |
| Integer |
| String |
| Float |
| Float |
| Integer |
Material | |
| String |
Machine | |
| String |
| String |
| String |
| String |
List of Modifiers
Modifiers can be used on any variable. Valid modifiers depend on the type of the variable.
Variable Type | Modifiers |
---|---|
String | U Uppercase Example: |
| L Lowercase Example:
|
Float | 00.00 Padding / Decimal Points
Example (For a 1.5101 diameter),
|
| F Fraction in inches Example (for an 1/8 inch diameter):
|
Tool Database - Remote Tool Databases
Users can share their own database via link sharing. Updates to the database (through our Cloud Upload functionality) can be downloaded by subscribers. Users can stop sharing their database at any point.
Share
To share your database, you must have first uploaded your local database through the cloud backup functionality in the tool database. Then go https://portal.vectric.com/toolDatabases and you should see your database there. You may see multiple entries for each version you have.
When you toggle the ‘share’ button, you will see a link which you can copy to the clipboard to share with others.
Update
Updating the database works in exactly the same way as the online backup. If you’ve chosen to share your database then subscribers will get the latest update that you upload so you don’t have to do anything extra here.
Subscribe
You can enter this dialog by using the ‘Remote Databases’ button to the right of the tool database selector on the Tool Database dialog.
Once you enter, you can enter the database URL supplied to you by copy-pasting into the URL field and clicking . This will download the Remote Database and will add it to the list.
As a subscriber, you will only be able to open those in read-only mode.
You can remove a Remote Database from your system be selecting the Database entry in the Remote Tool Database list and clicking .
Now in the main Tool Database Window you can select this Database from the Middle Dropdown menu to switch between them. Remote Databases are open in read-only (all settings will be greyed out and unchangeable).
- These tools can then be used in toolpaths, and edited with the Edit option in a toolpath as a normal tool.
- You can also right click tools in the Remote Database and copy them to your personal Databases for editing.
- Tools or groups can be exported into a separate tool database through the ‘Export’ button at the bottom.
This allows Shared machines to have a fixed Tool Database ready to go and be distributed easily. It allows users to share their databases and feeds & speeds with each other.
Your own database will remain unaffected and completely separate under the entry in the list called ‘Local’ unless you explicitly copy a tool to it.
Cut Operation
The Cut tool removes the selected objects from a design in a similar way to pressing the Delete key, but the selected objects are copied to the clipboard and can be Pasted into either the current file or a new file if required. Only one item can be Cut or Copied at a time.
Material Management
This dialog is used to edit and manage the list of materials for use in the tool database. It can be accessed through the Toolpaths Menu or the Tool Database dialog.
Material List
List the materials added to the database. Selecting a material activates it. This allows it to be edited in this dialog. In the Tool Database dialog, it results in switching the cutting data of the tools to be the set defined for the active material / machine (if any).
Add Material
Add a new material to the database and makes it active ready for editing.
Duplicate Material
Duplicates the active material and makes the new material active ready for editing.
Copy Cutting Data
This could optionally duplicate all the cutting data associated with the original material for all the tools so that there is a new set of cutting data for the new material as well.
Delete Material
Delete the active material and activate the next one up in the list.
Deleting Cutting Data
This is a destructive process deleting all the cutting data associated with this material across all the tools.
Name
Allows us to set the active material's name (if any). Two materials cannot have the same name.
Apply Changes
Apply changes by clicking or . Clicking will discard any changes made.
Female Inlay - Pocket
The Female Inlay - Pocket form offers all the same functionality of the Pocket Toolpath Form, but is automatically populated with corrected values. See the Pocket Tool documentation for more details.
Vector Selection Mode
When the Vector Selection Tool is chosen, the selected vectors are shown as dotted magenta lines. Vectors need to be selected before any of the editing tools such as scaling and moving etc. can be used.
Vector selection methods
Multiple vectors can be selected in the following ways:
- Manual multiple selection:
Hold down the Shift key while clicking the Left mouse button on each vector required. Objects can be deselected by simply clicking on the object again with a Shift key pressed. - Moving the cursor from Left to Right selects only fully enclosed objects:
Click and drag the left mouse button moving from Left to Right selects all objects completely inside the selection rectangle. - Moving the cursor from Right to Left selects all objects inside or touching the selection rectangle:
Click and drag the left mouse button moving from Right to Left selects all objects inside the selection rectangle + any that the selection touches. - Pressing the keyboard keys Ctrl+A will select all vector objects in the design:
Selected vectors are displayed as dotted magenta lines.
Deselecting Vectors
Selections can be cancelled by:
- Left clicking on an area outside the selection
- Pressing the Esc key
- Pressing the Right mouse button and clicking Selection ► Unselect All from the pop-up menu.
You must click on the white drawing background to get this option in the pop-up menu.
Migration Dialog
This tool helps existing users migrate their data from an older installation into the new version. You can migrate things like the Tool Database, Post-Processors in My_PostP
, Options and various Defaults.
- Copy Machine / Tool Database; This will migrate your tool database and machines and the post-processor associations. You can check the data from the Tool Database and Machine Configuration dialogs.
- Backup Tool Database Online; This will back up the new tool database (just migrated) to your online tool database backup area for the new version.
- My Post Processors; This will only copy your custom Post Processors in My_PostP folder.
- Options; Copy most of the options on Options Dialog.
- Custom Material Textures; For use in simulation and job setup.
- Sculpting Presets; Only in Aspire for use in the Sculpting tool.
Toolpath Tabs
The tab placement dialog allows you to place tabs either automatically or dynamically.
Add Tabs Automatically
Automatically place the tabs by setting the Tabs options and clicking the button
Specify Tabs
There are 2 options:
- Constant number - Attempts to add the specified number of tabs by distributing them evenly along the vectors.
- Constant distance between tabs - Attempts to add tabs at regularly spaced distances.
Placement
There are two options for placement of tabs. The first tab can be placed at the machining start point, using the corresponding option. Otherwise, the Avoid corners and curved regions option can be used. This option will try to avoid placing the tabs at corners, whilst still trying to use the options above which specify the number of tabs and the distance between them.
Note
It may not always be possible to avoid all corners, whilst trying to place the chosen number of tabs and have them spaced relatively evenly.
Interactive Tab Entry
You can interactively add tabs by clicking in the 2D view.
Add Tab
Click on the vector where no tab exists to insert a new tab.
Delete Tab
Click on an existing tab to delete it.
Move Tab
Click on the tab and drag to move it along the vector into the new position.
Delete All Tabs
Click the button to delete all of the tabs.
Calculation Edit Boxes
Numerical edit boxes generally support simple calculations.
A sum can be entered directly into the edit box:
Having typed an equation, pressing the = key will perform the entered calculation and fill the edit box with the answer.
Special Calculation Characters
As well as the simple numerical calculations, such as 3+(4/5), several of VCarve Desktop's stored values can be accessed by using certain letters (which are not case-sensitive): When used, VCarve Desktop substitutes the character with the appropriate value in the calculation.
Character | Name | Example | Description |
---|---|---|---|
W or X | Material Width |
| Half of the material width |
H or Y | Material Height |
| Twice the height of the material |
T or Z | Material Thickness |
| 0.25 units less than the material thickness |
P | PI (3.141593) |
| Area of a 10 radius circle (π.r2) |
I | Imperial Conversion |
| Converts 25.4mm to inches |
M | Metric Conversion |
| Converts 2 inches to millimetres |
' | Feet |
| 34 inches (2 feet and 10 inches) |
Import a Component or 3D Model
This command opens the File Open dialog window, and in Aspire allowing existing files (CRV3D extension for Aspire and CRV extension for VCarve) and importable 3rd party 3D files to be selected and opened. If you select a 3rd party 3D model format, the Orientate Model form will open (see below) to allow you to manipulate the 3D model before it is converted into a Component.
In VCarve Pro and VCarve Desktop, it allows for importable 3rd party 3D files to be selected and opened.
CRV3D | Note Aspire Only 3D data from files previously created and saved in ASPIRE will be opened and a new single Component Created (from all the visible 3D Components in the file when it was saved). The new Component will have the same name as the file. This will be imported at the size and position the part was saved in the original file. |
3DCLIP | Note Aspire Only 3D Clipart files are exported from Aspire. This format maintains the component structure of clipart pieces at the time of saving, so will import all the components comprising the clipart piece. This will be imported at the size and position the part was saved in the original file. |
V3M | V3M is a proprietary file format developed by Vectric for Vector Art 3D and Design and Make. Files in this format can be purchased from www.vectorart3d.com and www.designandmake.com and when imported into VCarve Desktop will create a new Component with the same name as the file. This will be imported at the size and position the part was saved in the original file. |
STL | This is a standard format for complex 3D models, based on a triangular mesh. STL files can be exported from many 3D design software programs such as Rhino. These models can be completely 3 dimensional (i.e. have a front, back, etc.), this means that when this type of file is opened that it must first be sized and oriented before a Component can be created (VCarve Desktop only represents base-relief so cannot work with a completely 3D object). Once the file becomes a Component it will have the same name as the original STL file. This file type will need to be imported using the Orientate 3D ModelVCarve Desktop. |
DXF | 3D DXF files from AutoCAD and many other CAD orientated modeling packages, these must be 3D meshes and not just wireframe data of the models vertices. This file type will need to be imported using the Orientate 3D ModelVCarve Desktop. |
3DS | A native format from 3D Studio Max and many other animation orientated modeling packages. This file type will need to be imported using the Orientate 3D ModelVCarve Desktop. |
OBJ | A native format from Wavefront and many other animation orientated modeling packages. This file type will need to be imported using the Orientate 3D ModelVCarve Desktop. |
SKP | A native format from the SketchUp modeling package. This file type will need to be imported using the Orientate 3D ModelVCarve Desktop. |
Note
If you wish to read data from a 3D digitizer or scanning device then STL is typically the best format that should be used to import the data. Many software packages that work with a scanner offer an STL export option, if not then a third party software program may be required to convert the data to an STL model.
Importing a 3D Model (STL, DXF, 3DS, OBJ, ...)
When one of these formats are chosen for 3D file Import, the imported model needs to be oriented and scaled before it can become a Component. A special import window is opened and a set of orientation/scaling tools enabled. Depending on the job type, import window will be different:
Re-Importing
Once a 3D Model has been imported then provided it has not been changed significantly it is possible to re-import the model to adjust the size, position, and slicing plane of the imported model. To re-import right click one of the components for the imported model in the component tree and select
File Types
CRV3D | Files previously created and saved in VCarve Desktop will be opened and displayed in the 2D Design window and 3D View if they contain 3D data. All calculated toolpaths are stored/opened from the CRV3D file. |
CRV | Files previously created and saved in VCarve Desktop will be opened and displayed in the 2D Design window. All calculated toolpaths are stored/opened from the CRV file. |
DXF | Files from other CAD or graphics software packages such as AutoCAD will be opened in the original size and position. The Job Setup Form is automatically opened showing the maximum X and Y dimensions of the opened design. The actual size of the material can then be specified along with the required thickness and appropriate X0, Y0 and Z0 origins. |
EPS | Files from typical design software such as Corel Draw can be opened. The Job Setup form will automatically be opened so the required material size can be specified. By default the EPS file will be placed with the lower left corner of the design at X0, Y0. |
AI | Files from typical design software such as Adobe Illustrator and Corel Draw can be opened. The Job Setup form will automatically be opened so the required material size can be specified. The AI file will be placed with the lower left corner of the design at X0, Y0 |
Software such as the Adobe product range can be used to convert files from other design and word processing software into the industry standard PDF file format. The text and vector content of PDF files is extracted when imported into VCarve Desktop. When importing multiple page PDF documents each page is placed on a separate layer. | |
SKP | SketchUp files with a .SKP extension (see www.sketchup.com) can be imported as 2D data suitable for machining. |
Smooth Components
Often it is advantageous to apply a general smoothing effect over the whole of a component (rather than smooth a particular area with the Sculpting Tools). To use this tool, select the components you wish to smooth and then click the Apply smoothing filter to selected components icon on the Modeling tab. The form will appear and VCarve Desktop will take a few seconds to prepare the model for the smoothing operation. You will see a progress bar at the bottom of the screen while it is doing this.
One or more Components can be selected for Smoothing. If you select multiple shapes or a Component Group then the software will need to Bake your selection into a single Component, if applicable you should ensure you have a safe copy of your current Components before proceeding.
If you wish to smooth individual components one after another, potentially with different amounts of smoothing, you can do this by selecting one component, apply a suitable smooth filter value with the slider and then hit the Bake Current Smoothing button in the form and then proceed to selecting the next component you wish to smooth. When pick a new Component the software may take a few seconds to pick it and apply the smoothing filter to it at the default of 50% strength. If you do not click on the button before you select a new component then the effects of the smoothing will be lost on the previously selected component.
Note
Smoothing should be performed with both the 2D and 3D View visible (Tile Windows), so you can easily see the selected Component in the 2D View and also view the effects of the smoothing in real time on the 3D model in the 3D View.
Smoothing
This slider will allow the user to control the strength of the smoothing applied to the Component. By default 50% smoothing is applied, using the slider different levels of smoothing can be applied to the model. Find the strength which gives you the amount of smoothing you require. If the Max setting has not smoothed the model enough then hit the Bake Current Smoothing button which resets the smoothing slider to allow you to do further smoothing.
Preserve Transparency
Checking ✓ this option will keep the smoothing only on the current 3D areas of the selected shapes and not smooth the edges into the background. Un-checking this option will smooth all the edges of the modeled area into the background of the part, blurring the silhouette of the Component.
Bake Current Smoothing
The button bakes the current smoothing value into the Component and resets the form. This means you are able to perform multiple smoothing operations without leaving the function.
3D Design and Management
As well as creating toolpaths directly from 2D drawings, VCarve Desktop can produce extremely flexible 3D toolpaths. These toolpaths are created from 3D design elements called 3D Components that can be generated from models created in external 3D design packages, imported as 3D clipart or built entirely from within VCarve Desktop using 2D artwork as a source.
The 3D View
The 3D View can show you the current Composite Model (which is built from all of the currently visible 3D Components and Levels), the Toolpath Preview (a highly accurate 3D simulation of the resulting physical object that will result from your toolpaths called the Preview Material Block). Which of these is currently displayed will depend on whether or not you have a part which has 3D Components and Toolpaths or are just working on something that only includes 2D Data.
Whenever you have the Preview Toolpaths form open on the Toolpaths tab, the 3D View displays the Preview Material Block instead of the Composite Model. When this is closed if you are working on a part that only includes 2D data and 2D or 2.5D toolpaths it will continue to display the Preview Material Block. If your part contains any visible 3D Components then as soon as the Preview Toolpaths form is closed it will revert to showing the Composite Model in the 3D View and hide the simulation. In addition to these items, you can see line drawings of any calculated toolpaths in the 3D View. The visibility of these calculated toolpaths can be controlled from the Toolpath List on the Toolpaths tab using the check-boxes next to the toolpaths name. If working in a 2 Sided environment you can view both sides of a project in the 3D View using the Multi Sided View option.
The Composite Model
VCarve Desktop has been designed to work in a way which enables the user to easily create even very complex projects. In any situation, the best approach to producing something complicated is to break it down into smaller pieces until a level of simplicity is reached that can be understood and managed. In VCarve Desktop this is achieved by letting the user work with pieces of the design which are combined to make the finished part. In the terminology of the software these pieces are called Components. To help organize the Components they are assigned to Levels. Step by step, Components and Levels can be created and modified until you have all the elements you need. In the images below you can see an example of how this might work. On the left you can see the separate component for a model of a bunch of grapes and on the right you can see these positioned to make the complete part - we call this resulting combination the Composite Model.
There is no limit to how simple or complex a Component or the Components on a Level can be (this is the user's choice). In the example shown, you can see that a model of a whole bunch of grapes may be made up of smaller individual components but they could also be combined to exist as one single Component (the assembled bunch of grapes) that could then be used to lay-out a more complex part with multiple bunches of grapes. They could also be organized so all the grapes were on one Level and leaf and stem on another to provide a different way of managing and manipulating the shapes. Each user will find a level of using Components and Levels they are comfortable with which may be dependent on the particular job or level of proficiency with the modeling tools.
3D Components and Levels
In VCarve Desktop, the aim is to end up with a set of Components and Levels that when combined together will make the finished 3D part. One way to think of this is like building a 3D collage or assembly. As the design evolves, new Levels or shapes may need to be created or existing ones changed. The parts of the collage are managed with the Component Tree which will be covered in more detail later.
Creating and Editing Components
An existing Component can be copied, scaled and have other edits carried out on it as an object. The user can also change the way it relates to the other Components, for instance whether it sits on top or blends into an overlapping area of another Component. The shape, location and relation of these pieces determine the look of the final part. As the job progresses, the user will need to create brand new Components or edit existing ones by adding new shapes, combining them with others or sculpting them.
Components can be created and edited by:
- Use a modelling tool to create shapes from 2D vectors.
- Import a pre-created 3D model - either a model previously created in Aspire or from another source such as a clipart library or a different modelling package.
- Create a 'texture' Component from a bitmap image.
- Use the Split Components Tool to break an existing Component into multiple pieces.
All of these methods are covered in detail throughout the training material.
Dynamic Properties
As well as having its underlying 3D shape, each component also has a number of dynamic properties that can be freely modified without permanently changing its true shape. These include scaling of the Component's height, the ability to tilt it, or to apply a graduated fade across it.
These dynamic properties can always be reset or altered at any time during your modeling process, which makes them a particularly useful way of 'tweaking 'your components as you combine them together to form your final composite model.
Combine Modes
The Combine Mode is a very important concept when working with 3D shapes within Aspire. The options for combine mode are presented when creating new shapes and also when deciding how Components and Levels will interact in the Component List. Rather than cover this in every section where it is applicable, it is worth summarizing the options here so the general concept can be understood.
When you have more than one 3D shape, such as the Component pieces of the design or where you have an existing shape and are creating a new one, then you need to have a way to tell the software how the additional entities will interact with the first. This can be an abstract concept for users who are new to 3D but it is an important one to grasp as early as possible. In Aspire this is controlled by a choice called the Combine Mode.
There are four options for this: Add, Subtract, Merge High, Merge Low.
As modeling is an artistic and creative process, there is no general rule to describe when to use each one. As a guide though you can assume that if the second shape's area is completely within the originals one then you will probably be adding or subtracting and if the shapes only partly overlap that you will probably use Merge or, very occasionally, Low.
The four options and their specific effects are described on the following pages. To illustrate the different effects a combination of an overlapping beveled square and a dome will be used. You can see in the image top right how these are arranged in the 2D View and how they overlap. Then you can see each individual shape in the images below middle and right. These shapes will be used to demonstrate the different Combine Modes. In every case the Dome will be considered the primary shape and the square is the secondary shape which is being combined with the first. In addition to the dome/square example some images of 'real world' parts will also be included to help to understand how these can be used on actual projects.
As well as working on individual shapes, the Combine Modes are also assigned to Levels. These will govern how the combination of all the individual components on one Level interacts with the result of all the Components on the Level below it in the Component Tree
Note:
There is a 5th Combine Mode available from the right mouse click menu after a component has been created called Multiply. This combine mode has specialist applications which are dealt with in the appropriate tutorial videos. This option will literally multiply the heights of the Component or Levels being combined to create the new Composite 3D shape.
Add
When Add is selected, it takes the first shape and then just adds the height of the second shape directly on top of the first. Any areas which overlap will create a shape which is exactly the height of each shape at that point added together (see below)
Typically the add option is mainly used when the shape being added sits completely within the original shape, this ensures that the uneven transition where the parts only partly overlap (as shown in the example) do not occur.
The example above shows the Maple Leaf and border extrusion Components being Added to the dome Component in the sign example from the Introduction to Modeling document.
Subtract
When Subtract is selected it takes the first shape and then removes the height of the second shape from the first. Any areas which overlap will be a combination of the original height/shape less the second shape. Areas where the shape goes into the background will become negative regions. You can see how this looks using the dome and square in the image below:
Typically subtract, like the add option, is mainly used when the shape being removed sits completely within the original shape, this ensures that the uneven transition where the parts only partly overlap (as shown in the example) do not occur.
The image shown above has some 'creases' to help define the muscles of the lioness. The shapes to create these recesses were created by using the Subtract option with the Create Shape tool on the vectors representing those recessed areas.
Merge
When the Merge option is selected any areas of the shapes which do not overlap remain the same. The areas that overlap will blend into each other so that the highest areas of each are left visible. This results in the look of one shape merging into the other and is in effect a Boolean union operation. You can see how this looks using the dome and square in the image below:
Typically the merge option is used when the shape being combined partly overlaps the original shape. This enables a reasonable transition to be made between them.
The image above shows 2 Herons, a rope border and banner Components. Each of these overlaps with the others and so they are set to Merge in this areas. Whatever is the higher of the two merged areas is what is prominent. In this case the rope is lower than everything and the Banner is higher than the Herons so the desired effect can be achieved.
Low
The Low option is only available when combining Components (not in the modeling tools). When this mode is selected, any areas which do not overlap are left as they were in the original two shapes. Any areas which overlap will create a new shape which is the lowest points taken from each shape, this is in effect a Boolean intersection operation. You can see how this looks using the dome and square in the image below:
The Low option is used for recessing a shape into a raised shape. An example of this is shown in the image above.
The example shown on the right above uses the Low option to combine the flat topped 'button' component on the left with the curved top face component with the letter 'A' on the right. Combining both components with the merge low option gives the keyboard button with the curved top you see in the bottom row.
Level Mirror Modes
Right-clicking Levels in the component tree will open a pop-up menu offering commands and operations related to the clicked level and Mirror Modes can be set in this way. If a mirror mode is set on a Level, all the components it contains will be continually mirrored dynamically as they are moved, transformed or edited. The mirroring is non-destructive, that is it can be turned off or on at any time and does not alter the underlying components in any permanent way. Working inside a Mirror modes Level is a simple way of achieving a complicated symmetrical pattern by editing only one half (or quarter, see below) of the design.
The available Mirror Modes are broadly divided into two groups. The first group apply one plane of symmetry:
- Left to Right
- Right to Left
- Top to Bottom
- Bottom to Top
These modes allow you to work in one half of your job and the other half will be automatically and dynamically generated for you. For example, in Left to Right mode you would place your components in the left half of your job and a mirrored equivalent of each would be created in the other half of the job. This 'reflection' is updated dynamically as you work.
The other group offer two planes of symmetry (horizontal and vertical):
- Top Left Quadrant
- Top Right Quadrant
- Bottom Left Quadrant
- Bottom Right Quadrant
When using these modes your components should all be in the quadrant (quarter) of the job. Mirrored reflections horizontally and vertically will be created in the other quadrants of the job for you.
Multi Sided View
When working in a 2 Sided environment you can create components independently per side or using the Right click option you can copy or move a component to the opposite side. Selecting the option to work in 'Multi Sided View' allows you to view components you may have on the Top and Bottom side in the 3D View. In the Toolpath Preview form of a project that contains toolpaths for the Top and Bottom Sides the multi sided view presents the simulation of the toolpath preview on both sides also, if the multi sided view is not selected you can use the 'Preview all Sides' option in the Toolpath Preview form to display the Top and Bottom Toolpaths in the 3D view. 2 Sided Setup will be described in detail later in the relevant section of this manual.
Kickstarter Wizard
The Kickstarter Wizard is provided to assist with the selection of a machine configuration, when you first use the software.
You can access the Kickstarter wizard at any time, by selecting Help > Kickstarter Wizard from the main menu bar of VCarve Desktop
The wizard has multiple pages to take you through,
- Signing in
- Registering your VCarve Desktop software in V&Co
- Looking for your machine online
- Manual configuration of your machine
Post-Processor Editing
What does the Post Processor Do?
The post processor is the section of the program that converts the XYZ coordinates for the tool moves into a format that is suitable for a particular router or machine tool. This document details how to create and edit the configuration files that customize the output from the program to suit a particular machine control.
Below are sections of a typical program that has been post processed into both G-Code and HPGL
G-Code Output
T1 M6
G17
G0 Z4.5000
G0 X0.0000 Y0.0000 S12000 M3
G0 X2.4567 Y7.8342 Z0.2500
G1 Z-0.0500 F5.0
G3 X3.3784 Y8.7559 I0.0000 J0.9218 F66.0
G3 X2.4567 Y9.6777 I-0.9218 J0.0000
G3 X1.5349 Y8.7559 I0.0000 J-0.9218
HPGL Output
IN;PA;
PU2496,7960;
PD2496,7960;
AA2496,8896,90.000
AA2496,8896,90.000
AA2496,8896,90.000
AA2496,8896,90.000
PU2496,7960;
PU2496,6096;
Machine controller manufacturers will often customize the file format required for programs to run on a particular machine in order to optimize the control to suit the individual characteristics of that machine.
The Vectric post processor uses simple text based configuration files, to enable the user to tailor a configuration file, should they wish to do so.
Post Processor Sections
Vectric post processors are broken down into sections to aid clarity, try to write your post processors in a similar style to aid debugging.
File Comments
A section where you can describe the post processor and record any changes to the post processor, each line is a comment and starts with a ‘+’ character or a ‘|’ character.
+ History
+ Who When What
+ ======== ========== ===========================
+ Tony 14/07/2006 Written
+ Mark 26/08/2008 Combined ATC commands, stop spindle on TC
+================================================
Global File Statements
Statements are items that are either used only once, or have static values throughout the file. Write statement names in upper case letters for clarity.
Statement | Result |
---|---|
| The name that will appear in the post processor list |
| The file extension that the file will be given |
| The units that the file outputs (INCHES or MM) |
| The machine tool manufacturer has supplied a driver (usually a printer driver) thatn can directly accept the NC file output (For example see Generic HPCL_Arcs.pp) |
| Indicates that plunge moves to Plunge (Z2) height (that is set on the material setup form) are rapid moves |
| The control software uses a document interface that can directly accept the NC file output. |
| The moves in the Y axis are to be wrapped around a cylinder of the specified diameter. The "Y" values will be output as "A" |
| The moves in the X axis are to be wrapped around a cylinder of the specified diameter. The "X" values will be output as "B" |
| Spindle speed for this machine is output as a range of integer numbers between 1 and 15 representing the actual speed in RPM of the spindle, (between 4500 and 15000 RPM in the quoted example). For an example, see the file: Roland_MDX-40_mm.pp |
| This command allows you to substitute a character output within the variables (such as The characters are entered in pairs, Original - Subsititued. For example MACH 3 control software uses parentheses as comment delimiters, and does not allow nested comments. Most tools within the Vectric Tool Database have parentheses within the “Name” section; if these names are output, this would cause an error within Mach3. The command |
| Rotary: Enables / Disables output of the feedrate F in Inverse Time Feed Mode. In this mode, we're expected to complete a move in one divided by the F number of minutes. In GCode, this would usually be a G93 to switch on Inverse Time Mode, or a G94 to set Units per Minutes mode. |
| Indicates that this post-processor supports laser toolpaths (if the Laser Module is installed). |
| Optional minimum arc radius. Arcs which have a radius smaller than this value will be replaced with a single straight line move. |
| Optional maximum arc radius. Arcs which have a radius greater than this value will be polygonized. |
POST_BASE | This is a no longer supported way of inheriting the content of another post-processor. See the POST_BASE Migration page for more details. |
Tape Splitting Support
A section that describes how a long toolpath output will be split:
TAPE_SPLITTING=MAX_NUM_LINES LINE_TOL "FILENAME_FORMAT" START_INDEX INDEX_ON_FIRST_FILE
For example a command of:
TAPLE_SPLITTING=1000 100 "%s_%d.tap" 1 "YES"
would lead to...
Output will be split into multiple files of a maximum of 1000 lines (+ however many lines in there are within the footer section of the post processor), if a retract move exists after line 900 (1000 – 100), the file will be split at that move. If the file was called "toolpath" the split files would be named toolpath_1.tap, toolpath_2.tap etc. The first toolpath output will be "toolpath_ 1.tap" there will be no file named "toolpath" without an index number, (as INDEX_ON_FIRST_FILE= YES
is used), unless the file was less than 1000 lines long, in which case the file would not be split.
Note
Some controllers that require NC files to be split, also have limitations on the number of characters within a filename. For example they may require the file to be named with the MSDOS style 8.3 filename format. This should be considered when naming the output file.
Line Terminating Characters
LINE_ENDING="[13][12]"
Decimal values of the characters appended to each separate line of the post processed file. (Will usually be [13][10]) (Carriage return, line feed) for any controller that can read a windows or MSDOS format text file.
Block Numbering
If you wish to add line numbers to the output file, the current line number is added with the variable [N]. The behaviour of this line number variable is controlled by the following variables:
Statement | Result |
---|---|
| Value at which the line numbering should start |
| Incremental value between line numbers |
| The maximum line number to output, before cycling to the Important - Some controllers have a limit to the number of lines that can be displayed on the control |
Variables
Variable Name | Output using | Value | Example File |
---|---|---|---|
|
| Current Feed Rate. | Mach2_3_ATC_Arcs_inch.pp |
|
| Current Cut Feed Rate. | CNCShark-USB_Arcs_inch.pp |
|
| Current Plunge Feed Rate. | CNCShark-USB_Arcs_inch.pp |
|
| Current Spindle Speed in R.P.M. | GCode_arc_inch.pp |
|
| Current power setting for jet-based tools (e.g. lasers) | grbl_mm.pp |
|
| Current Tool Number. | Mach2_3_ATC_Arcs_inch.pp |
|
| Previous Tool Number. | NC-Easy.pp |
|
| Line Number. | Mach2_3_ATC_Arcs_inch.pp |
|
| Name of Current Tool. | MaxNC_inch.pp |
|
| Text from Note field in ToolDB for current tool | Busellato_Jet3006_arc_inch.pp |
|
| Name of Current Toolpath. | Viccam_ATC_Arcs_inch.pp |
|
| Filename (Produced by “Save Toolpath(s)”). | ez-Router_inch.pp |
|
| Folder Toolpath File was saved to. | Woodp_arc_mm.pp |
|
| Toolpath File Extension. | TekcelE_Arc_ATC_3D.pp |
|
| Toolpath Folder Pathname. | WinPC-NC_ATC_Arcs_mm.pp |
|
| Current coordinate of tool position in X axis. | GCode_arc_inch.pp |
|
| Current coordinate of tool position in Y axis. | GCode_arc_inch.pp |
|
| Current coordinate of tool position in Z axis. | GCode_arc_inch.pp |
|
| Current coordinate of tool position in A axis. | |
|
| Arc centre in X Axis (relative to last X,Y position). | Mach2_3_ATC_Arcs_inch.pp |
|
| Arc centre in Y Axis (relative to last X,Y position). | Mach2_3_ATC_Arcs_inch.pp |
|
| Arc centre in X Axis (absolute coordinates). | Isel_arc_mm.pp |
|
| Arc centre in Y Axis (absolute coordinates). | Isel_arc_mm.pp |
|
| Start position of an arc in X axis. | TextOutput_Arcs_mm.pp |
|
| Start position of an arc in Y axis. | TextOutput_Arcs_mm.pp |
|
| Mid-point of arc in X (absolute coordinates). | TextOutput_Arcs_mm.pp |
|
| Mid-point of arc in Y (absolute coordinates). | TextOutput_Arcs_mm.pp |
|
| Mid-point of arc in X (incremental coordinates). | TextOutput_Arcs_mm.pp |
|
| Mid-point of arc in Y (incremental coordinates). | TextOutput_Arcs_mm.pp |
|
| The radius of an arc. | Bosch_ATC_Arcs_mm.pp |
|
| The angle of an arc. | Generic HPGL_Arcs.pp |
|
| Home tool position for X axis. | CAMTech_CMC3_mm.pp |
|
| Home tool position for Y axis. | CAMTech_CMC3_mm.pp |
|
| Home tool position for Z axis. | CAMTech_CMC3_mm.pp |
|
| Safe Z Height / Rapid Clearance Gap. | EMC2 Arcs(inch)(*.ngc) |
|
| Diameter of cylinder that axis is wrapped around. | Mach2_3_WrapY2A_ATC_Arcs_mm.pp |
|
| Length of material in X. | Mach2_3_ATC_Arcs_inch.pp |
|
| Length of material in Y. | Mach2_3_ATC_Arcs_inch.pp |
|
| Length of material in Z. | Mach2_3_ATC_Arcs_inch.pp |
|
| Minimum value of material in X. | MaxNC_inch.pp |
|
| Minimum value of material in Y. | MaxNC_inch.pp |
|
| Minimum value of material in Z. | MaxNC_inch.pp |
|
| Maximum value of material in X. | MaxNC_inch.pp |
|
| Maximum value of material in Y. | MaxNC_inch.pp |
|
| Maximum value of material in Z. | MaxNC_inch.pp |
|
| Origin Position in X. | TextOutput_Arcs_mm.pp |
|
| Origin Position in Y. | TextOutput_Arcs_mm.pp |
|
| Z Zero Position, Table or Material Surface. | TextOutput_Arcs_mm.pp |
|
| X, Y Origin. | TextOutput_Arcs_mm.pp |
|
| List of tools used (In order of use). | Mach2_3_ATC_Arcs_inch.pp |
|
| List of toolpaths used in file (in order of use). | Mach2_3_ATC_Arcs_inch.pp |
|
| Toolpath Notes (Toolpath Control form). | Mach2_3_ATC_Arcs_inch.pp |
|
| File Notes (Edit > Notes). | Mach2_3_ATC_Arcs_inch.pp |
|
| File creation time. | Mach2_3_ATC_Arcs_inch.pp |
|
| File creation date. | Mach2_3_ATC_Arcs_inch.pp |
|
| Dwell time in seconds when drilling. | Mach2_3_Arcs_inch.pp |
|
| Name of the product used to output file, including version number. | |
|
| Tool diameter. | |
|
| Rotary: Current Inverse Time Rate | AvidCNC_WrapX2A_G93_inch.pp |
Format of Variables
Values for tool position, feed rates, spindle speeds etc. are inserted into the file using variables. Variables are used throughout the file; the variables are replaced with the current value for that item when the file is post processed. For example, the current X, Y and Z tool positions at any time, are inserted into the file by using the variable output, [X]
, [Y]
and [Z]
respectively.
Write variable names in upper case letters for clarity.
A Variable is formatted as follows:
VAR VARIABLE = [VO|WO|CS|VF|MX]
where
VO
= Variable output for example X, XF or F.WO
= When output, A=Always, C=Only when changed.CS
= Character string output before value .VF
= Value format, determines the format that the value is output with.MX
= Multiplier Value.
A typical variable
1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | 9 | 10 | 11 | 12 | 13 | 14 | 15 |
---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
VAR
- This line is a Variable.- Variable Name.
- Equals Sign.
- Open Square bracket - (start of variable formatting parameters).
- Variable label - i.e. label that is substituted with the variable value.
- Vertical Bar - Parameter separator.
A
= Always output value,C
= Only output value when it changes- Vertical Bar - Parameter separator.
- Character string to print before variable value.
- Vertical Bar - Parameter separator.
- Optional Format Flags - for details see below.
- Value Format - units and number of decimal places to output.
- Vertical Bar - Parameter separator.
- Output multiplier - for details see below.
- Close Square Bracket - End of formatting parameters.
Formatting the Output Value
The values format string should be formatted as follows:
FORMAT_FLAGS FIELD_WIDTH DECIMAL_SEPARATOR DECIMAL_PLACES
The format flags are optional and only needed by a small number of controllers they will be described shortly.
Field Width The Field width represents the minimum number of characters that are output. The field width is usually set to “1” a value greater than 1 is typically only required if a controller expects to see a fixed number of characters for the value. If this is the case, a number greater than 1 can be entered. The number entered will ensure that that number of characters is output. The number that represents the field width includes the full floating-point number for the output value, (including the decimal separator character).
Decimal Separator The decimal separator character is almost always just a period character, but there are some controllers that expect to see a comma character. (For an example of a post processor that does not use a period character, see the file: Heidenhain_inch.pp)
Decimal Places The number of decimal places output following the decimal separator. The values are often set at 3 for controllers operating in Metric, or 4 for controllers operating in Inches.
Optional Format Flags
The output values can be further modified by using the optional format flags:
Flag | Function | Default (without flag) |
---|---|---|
| Left Justify the output | Values are right justified |
| Prefix the value with '+' or '-' | Only negative values are prefixed |
| If value has fewer characters than the set minimum, the value is prefixed with zeroes | Values is prefixed with blanks spaces |
| Values is always output with a separator character ( in practice this would only change the output value if the value is set to output integer values only) | When output is set to integer only, separator charactor is not appended to value. |
Default Formatting For Variables
Most variables have a default format; (shown below) to set a different format for a variable, enter the line below in your post processor and alter the parameters to suit your controller.
Default | Example |
---|---|
|
The line number will always be output. An 'N' character will be inserted before the line number. It will be output as an integer number |
|
The spindle speed will always be output. An 'S' character will be inserted before the value and it will be output as an integer number. |
|
The feed rate will be output with an F character before the value, and will only be output when it changes. The value will be output to 1 decimal place Note In this format string there is an option extra parameter. This is the value multiplier. |
VAR PLUNGE_RATE = [FP|A||1.0] |
The plunge rate will be output with an F character before the value, and will only be output when it changes. The value will be output to 1 decimal place. Note In this format string there is an option extra parameter. This is the value multiplier. |
|
The cut rate will be output with an F character before the value, and will only be output when it changes. The value will be output to 1 decimal place. Note In this format string there is an option extra parameter. This is the value multiplier. |
|
The position value will be output with an ‘X’ character before the value, the position will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The home position value will be output with an ‘X’ character before the value, the position will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with an ‘X’ character before the value, the position will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
Note In this format string there is an option extra parameter. This is the value multiplier. |
|
The value will be output with an ‘Y’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with a ‘J’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with a ‘J’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
Note In this format string there is an option extra parameter. This is the value multiplier. |
|
The value will be output with a ‘X’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with a ‘X’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with a ‘R’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with a ‘A’ character before the value, the value will Always be output, and will be output to 3 decimal places, this would typically be suitable for a control that requires metric output. If you wished to output the values to 4 decimal places as would be more typical for a controller operating in inches. You would format the line as follows.
|
|
The value will be output with an ‘X’ character before the value, the value will Always be output, and will be output to 3 decimal places. |
Multiplier Value
The multiplier value is used to multiply the value to output a different value. Common reasons for wishing to do this are:
To convert the default output of an Inch post processor, from inches per minute to inches per second, (Multiply by 0.01666).
To convert the default output of a Metric post processor, from mm per minute to mm per second, (Multiply by 0.0166).
To make positive values negative (and vice versa), (Multiply by -1).
To convert the output of an arc angle from radians to degrees, (Multiply by 57.2957795).
To multiply or divide by a fixed factor (I.E. produce 1:4 scale model, Multiply by 0.25)
Post Processor Blocks
HEADER
+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------
begin HEADER
"Commands"
The header is the location for the instructions that are output once, at the start of the file, these generally setup modal commands for the controller.
For example, the Header might contain a command to display the filename on the controller and a series of “G-Codes” to set the machine up, for instance G20 to tell the control that the moves are in inches, or G21 to tell the control that the moves are in millimetres.
Variables that you might wish to be within the header section, could include:
Information about the Material Block
- Minimum extent in X = [XMIN]
- Minimum extent in Y = [YMIN]
- Minimum extent in Z = [ZMIN]
- Maximum extent in X = [XMAX]
- Maximum extent in Y = [YMAX]
- Maximum extent in Z = [ZMAX]
- Length of material in X = [XLENGTH]"
- Length of material in Y = [YLENGTH]"
- Depth of material in Z = [ZLENGTH]"
Home Position Information
- Home X = [XH]
- Home Y = [YH]
- Home Z = [ZH]
- Rapid clearance gap or Safe Z = [SAFEZ]
Details of the first tool to be used.
- Tool Number = [T]
- Tool name = [TOOLNAME]
Initial cutting speeds
- Feed Rate used for cutting and plunging into the material = [F]
- Feed Rate whilst tool is Cutting the material = [FC]
- Feed Rate whilst tool is plunging into the material = [FP]
Actual values depend on the UNITS set (see Global File Settings) Defaults are either MM/Minute or Inches/Minute, but the output can be changed to suit by setting the appropriate “VAR FEED_RATE” formatting.
Spindle Speed
- Spindle Speed = [S] R.P.M.
SPINDLE_ON
+---------------------------------------------------
+ Commands output at when the Spindle first turns on.
+---------------------------------------------------
begin SPINDLE_ON
"Commands"
The Spindle On section was added to allow for Spindle and Laser operations in the same Post Processor instead of having the Spindle on command as part of the header.
Typically this will just have the Spindle on command (M03 for example) but can also include a Spindle speed command [S]
TOOLCHANGE
+---------------------------------------------------
+ Commands output at toolchange
+---------------------------------------------------
begin TOOLCHANGE
"Commands"
Commands that are output when a change of tool is required. Variables and commands that might be used include:
- Previous Tool Number = [TP]
- Tool Number = [T]
- Tool name = [TOOLNAME]
- Toolpath Name = [TOOLPATH_NAME]
- Toolpath Pathname = [PATHNAME]
- Toolpath File Name = [TP_FILENAME]
- Toolpath File Directory = [TP_DIR]
- Toolpath Extension = [TP_EXT]
- Spindle Speed = [S] R.P.M.
- M3 M Code often used to turn spindle on (Clockwise rotation).
- M5 M Code often used to turn spindle off.
NEW_SEGMENT
+---------------------------------------------------
+ Commands output for a new segment ( new toolpath with current toolnumber)
+---------------------------------------------------
begin NEW_SEGMENT
"Commands"
For an example of a NEW_SEGMENT section, see the file: Mach2_3_ATC_Arcs_inch.pp
Commands that are output when a new toolpath uses the currently selected tool, but perhaps a different spindle speed is required or the machine requires additional instructions.
Any commands that are used in the NEW_SEGMENT section should not need to be included within the TOOLCHANGE section as a tool-change will also automatically call the instructions in the NEW_SEGMENT section.
Variables that are commonly used include.
- Spindle Speed = [S] R.P.M.
- M3 M Code often used to turn spindle on (Clockwise rotation).
- M5 M Code often used to turn spindle off.
INITIAL_RAPID_MOVE
+---------------------------------------------------
+ Commands output for Initial rapid move
+---------------------------------------------------
begin INITIAL_RAPID_MOVE
"Commands"
For an example of a INITIAL_RAPID_MOVE section, see the file: Saom_OSAI_Arc_inch.pp
Commands that are output when the very first rapid move is made following the header or a tool change. A Section not used for most posts, but useful if the very first rapid move, needs to output different information to subsequent rapid moves. This section is sometimes required for HPGL variants.
RAPID_MOVE
+---------------------------------------------------
+ Commands output for rapid moves.
+---------------------------------------------------
begin RAPID_MOVE
"Commands"
Commands that are output when rapid moves are required.
FIRST_FEED_MOVE
+---------------------------------------------------
+ Commands output for first feed rate move in a series of feed moves.
+---------------------------------------------------
begin FIRST_FEED_MOVE
"Commands"
This section is commonly used where controllers require that the Feed Rate is set at the first feed move, this rate would then be used for subsequent cut moves.
For an example of a FIRST_FEED_MOVE section, see the file: Axyz_Arcs_ATC_inch.pp
FEED_MOVE
+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------
begin FEED_MOVE
"Commands"
Used to output information required at every move, or all feed moves except for the First Feed Move, if a FIRST_FEED_MOVE section is present within the post processor.
FIRST_CW_ARC_MOVE
+---------------------------------------------------
+ Commands output for the first clockwise arc move in a series of cw arc moves
+---------------------------------------------------
begin FIRST_CW_ARC_MOVE
"Commands"
Similar to the FIRST_FEED_MOVE section, but for clockwise arc segments. This section is commonly used where controllers require that the Feed Rate is set for the first arc segment, this rate would then be used for subsequent arc moves in the same direction.
For an example of a FIRST_CW_ARC_MOVE section, see the file: Centroid_Arcs_inch.pp
FIRST_CW_HELICAL_ARC_PLUNGE_MOVE
+---------------------------------------------------
+ Commands output for clockwise helical arc plunge move in a series of moves.
+---------------------------------------------------
begin FIRST_CW _HELICAL_ARC_MOVE
"Commands"
Similar to the FIRST_CW_ARC_MOVE section, but for moves that also move in Z. Feed rates output are from Plunge rate set for the tool.
For an example of a CW_HELICAL_ARC_PLUNGE_MOVE section, see the file: Mach2_3_ATC_Arcs_inch.pp
FIRST_CW_HELICAL_ARC_MOVE
+---------------------------------------------------
+ Commands output for clockwise helical arc move in a series of moves.
+---------------------------------------------------
begin FIRST_CW_HELICAL_ARC_MOVE
"Commands"
Similar to the FIRST_CW_ARC_MOVE section, but for moves that also move in Z.
For an example of a CW_HELICAL_ARC_MOVE section, see the file: Mach2_3_ATC_Arcs_inch.pp
CW_ARC_MOVE
+---------------------------------------------------
+ Commands output for clockwise arc moves.
+---------------------------------------------------
begin CW_ARC_MOVE
"Commands"
Similar to the FEED_MOVE section, but for clockwise arc segments.
For an example of a CW_ARC_MOVE section, see the file: Centroid_Arcs_inch.pp
CW_HELICAL_ARC_MOVE
+---------------------------------------------------
+ Commands output for clockwise helical arc moves
+---------------------------------------------------
begin CW_HELICAL_ARC_MOVE
"Commands"
Similar to the CW_ARC_MOVE section, but for moves that also move in Z.
For an example of a CW_HELICAL_ARC_MOVE section, see the file: Mach2_3_ATC_Arcs_inch.pp
FIRST_CCW_ARC_MOVE
+---------------------------------------------------
+ Commands output for the first counter-clockwise arc move in a series of ccw arc moves.
+---------------------------------------------------
begin FIRST_CCW_ARC_MOVE
"Commands"
Similar to the FIRST_FEED_MOVE section, but for counter-clockwise arc segments. This section is commonly used where controllers require that the Feed Rate is set for the first arc segment, this rate would then be used for subsequent arc moves in the same direction.
For an example of a FIRST_CCW_ARC_MOVE section, see the file: Centroid_Arcs_inch.pp
FIRST_CCW_HELICAL_ARC_PLUNGE_MOVE
+---------------------------------------------------
+ Commands output for counter- clockwise helical arc plunge move in a series of moves.
+---------------------------------------------------
begin FIRST_CCW_HELICAL_ARC_MOVE
"Commands"
Similar to the FIRST_CCW_ARC_MOVE section, but for moves that also move in Z. Feed rates output are from Plunge rate set for the tool.
For an example of a CCW_HELICAL_ARC_PLUNGE_MOVE section, see the file: Mach2_3_ATC_Arcs_inch.pp
FIRST_CCW_HELICAL_ARC_MOVE
+---------------------------------------------------
+ Commands output for first counter-clockwise helical arc move in a series of moves.
+---------------------------------------------------
begin FIRST_CCW_HELICAL_ARC_MOVE
"Commands"
Similar to the FIRST_CCW_ARC_MOVE section, but for moves that also move in Z.
For an example of a CCW_HELICAL_ARC_MOVE section, see the file: Mach2_3_ATC_Arcs_inch
CCW_ARC_MOVE
+---------------------------------------------------
+ Commands output for counter-clockwise arc moves.
+---------------------------------------------------
begin CCW_ARC_MOVE
"Commands"
Similar to the FEED_MOVE section, but for counter-clockwise arc segments.
For an example of a CCW_ARC_MOVE section, see the file: Centroid_Arcs_inch.pp
CCW_HELICAL_ARC_MOVE
+---------------------------------------------------
+ Commands output for counter-clockwise helical arc moves
+---------------------------------------------------
begin CCW_HELICAL_ARC_MOVE
"Commands"
Similar to the CCW_ARC_MOVE section, but for moves that also move in Z.
For an example of a CCW_HELICAL_ARC_MOVE section, see the file: Mach2_3_ATC_Arcs_inch.pp
FOOTER
The footer is the section of the post processor for instructions that are sent to the controller at the end of a file. These might be instructions to return the tool to the home position, switch the spindle off or switch the power off to the drives.
+---------------------------------------------------
+ Commands output at the end of the file
+---------------------------------------------------
begin FOOTER
"Commands"
Variables that are commonly used include.
- G00 [XH] [YH] [ZH] Rapid to X,Y,Z Home position.
- M05 M Code often used to turn spindle off.
- M30 M Code often used to signify the end of the file.
Jet Support Sections
These sections are for supporting jet-based cutting tools such as lasers, plasmas and waterjets.
JET_TOOL_POWER
+---------------------------------------------------
+ Commands output when the cutter's power is set
+---------------------------------------------------
begin JET_TOOL_POWER
"Commands"
For an example of a JET_TOOL_POWER section, see the file: Grbl.pp
Commands that are output when the power setting associated with a laser 'tool' is issued.
JET_TOOL_ON
+---------------------------------------------------
+ Commands output when the cutter's power is turned ON
+---------------------------------------------------
begin JET_TOOL_ON
"Commands"
For an example of a JET_TOOL_ON section, see the file: Grbl.pp
Commands that are output when the jet tool is powered on. This is broadly equivalent to SPINDLE_ON, but is typically issued a the end of a plunge move when the jet cutter is already at the intended cutting height, instead of before the plunge move as required by a spindle based cutter.
JET_TOOL_OFF
+---------------------------------------------------
+ Commands output when the cutter's power is turned OFF
+---------------------------------------------------
begin JET_TOOL_OFF
"Commands"
For an example of a JET_TOOL_OFF section, see the file: Grbl.pp
Commands that are output when the jet tool is powered off.
Other Less Frequently Used Sections
FEED_RATE_CHANGE
+---------------------------------------------------
+ Commands output when feed rate changes
+---------------------------------------------------
begin FEED_RATE_CHANGE
"Commands"
For an example of a FEED_RATE_CHANGE section, see the file: Gravograph_IS200.pp
Commands that are output when the feed rate is changed. This section is not often used as many controllers will accept feed rate changes appended to other instructions, but sometimes used with HPGL variants.
FIRST_PLUNGE_MOVE
+---------------------------------------------------
+ Commands output for the First Plunge Move, in a series of plunge moves.
+---------------------------------------------------
begin FIRST_PLUNGE_MOVE
"Commands"
For an example of a FIRST_PLUNGE_MOVE section, see the file: Holz-Her_7123_ATC_Arcs_mm.pp
This section is often used on machines that do not fully support simultaneous 3D movement, for example the Z Axis cannot travel as fast as the X & Y Axis. Another use of this section might be to include commands that you wish to output whenever the first plunge move occurs. For example, commands to switch on a plasma torch. Multiple plunges would normally only be output within a ramping move, so this command would be useful for controls that automatically rapid between cuts and where instructions such as revised speeds and feed need to be specified on the first plunge move and these instructions are not required for subsequent plunge moves within the ramping operation.
PLUNGE_MOVE
+---------------------------------------------------
+ Commands output for Plunge Moves
+---------------------------------------------------
begin PLUNGE_MOVE
"Commands"
For an example of a PLUNGE_MOVE section, see the file: Burny_arc_inch.pp
This section is often used on machines that do not fully support simultaneous 3D movement, for example the Z Axis cannot travel as fast as the X & Y Axis. Another use of this section might be to include commands that you wish to output whenever a plunge move occurs. For example, commands to switch on a plasma torch.
RETRACT_MOVE
+---------------------------------------------------
+ Commands output for Retract Moves
+---------------------------------------------------
begin RETRACT_MOVE
"Commands"
For an example of a RETRACT _MOVE section, see the file: Burny_arc_inch.pp
A use of this section might be to include commands to switch off a plasma torch.
DWELL_MOVE
+---------------------------------------------------
+ Commands output for Dwell Commands
+---------------------------------------------------
begin DWELL_MOVE
"Commands"
For an example of a DWELL_MOVE section, see the file: Mach2_3_Arcs_inch.pp
This command was introduced for VCarve Pro 7.5 and Aspire 4.5 and later. It is used with a drilling toolpath, when a Dwell time has been specified in the program. If this section is not defined any dwell commands are ignored, but the rest of the drilling toolpath will be output as normal. The DWELL variable is documented in the Variables section.
Special Characters
Most characters can be output within the confines of the post processor output statements; however, certain characters have special meaning within the post processor configuration files and cannot be output directly.
These are, the Square brackets [ ], and the double quote character “ It may be the case that you need to output one of these characters within your output file.
If you wish to output one of these characters, you can do so by enclosing the decimal equivalent of the ASCII value of the special character that you wish to output, within square brackets, as shown below. This method can also be used to insert any ASCII value, even non-printable characters.
- [91] Outputs a left hand square bracket.
- [93] Outputs a right hand square bracket.
- [34] Outputs a double quote character.
- [13] Outputs a carriage return.
- [10] Outputs a line feed.
For an example of a file that uses special characters, please see: Biesse_Rover_Arcs_mm.pp
Example: Adding Tool-Change Commands
For the majority of cases, the quickest and easiest way of producing a customised post processor to suit your controller, will be to edit an existing post processor. To do this, first create a simple test file that you can use to test the output of your post processor. A simple file might consist of a line, and two circles. Produce a shallow cutting profile toolpaths for each of the shapes, machining “On” the line, “Inside” one of the circles and “Outside” the other circle.