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.

The size forms may be limited

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).

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.

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

Tool Properties are divided into two categories,

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

Apply Changes

If you modify the Tool database, your changes will only be saved if you click OK. If you exit the Tool Database window using the Cancel button, any changes you have made since opening the Database will be discarded.

Tool Tree

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

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

New Tool

Create a new tool with the default name for its type. The tool will be created with the first available type by default, but that can be changed through the Tool Type dropdown to the desired type.

Copy Tool

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

The cutting parameters can be subsequently be:

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

Delete Tool

Delete the tool as well as all of the cutting data for all machines / materials for which it was defined. If we're deleting a group, this will delete all the tools inside it in the same way.

New Tool Group

Create a new group in the tool database. Tools can then be dragged inside the newly created group. Alternatively, select the group and create a new tool directly under the selected group.

Export Tools

Export an individual tool or an entire group to a tool database file.

Import Tools

A tool database file can be imported into the currently open tool database. You will have 3 options,

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

Tool Definition

When a tool or group is selected in the Tool List, its properties are displayed in the Tool Info section on the right-hand side of the Tool Database.

Name

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

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

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

Tool Type

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

test
V-Bit
test
Engraving
test
Tapered Ball Nose
test
Ball Nose
test
End Mill
test
Radiused End Mill
test
Form Cutters
test
Diamond Drag
test
Drills

Notes

The tool notes section simply allows you to save any additional text descriptions, special instructions or relevant information you may require, within your tool definition.

Diameter

The diameter of the tool in either inches or mm. The tool image will indicate where this dimension is taken from.

Number of Flutes

The number of Flutes for the bit. This is particularly useful if you would like to calculate a Chip Load value.

Cutting Data

The cutting data is the set of parameters which can differ between materials and machines. This set of parameters are defined to be per machine per material. The visible set of parameters are the ones for the active material / machine.

Creation / Copying

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

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

Pass Depth

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

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

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

Stepover

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

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

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

Final Pass Stepover

The distance the cutter moves over when finish machining and is usually set to be a relatively small distance to produce a smooth surface finish on the job.

Clearance Pass Stepover

Only used when a V-Bit tool is being used to rough machine at multiple Z levels down to a specified flat depth. This stepover can be much larger than the Final Pass Stepover because the tool is only rough machining material away. Increasing the Clearance Pass Stepover will reduce the machining time, but you must be careful to ensure it is not too great for the material being cut.

Spindle Speed

Speed of tool rotation, specified in revolutions per minute.

Feed Rate

The surface cutting rate at which the cutter is moved in the material. The units can be specified in distance per second or minute.

Plunge Rate

The cutting rate at which the cutter is moved vertically into the material or during ramping moves. The units can be specified in distance per second or per minute.

Material / Machine

The Feed rate and Plunge rate you should use will vary depending upon the material being machined and the tooling being used.

Chip Load

This is the calculated Chip Load based on the entered values for the Number of Flutes, Spindle Speed and Feed Rate. This is displayed to conveniently be able to compare it with manufacturer-recommended Chip Load Values.

Maximum Burn Rate

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

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

Tool Number

This is the number of the tool needed to machine the job. When using a CNC machine with an Automatic Tool Changer (ATC), it is critical that the correct tool required to cut the job is located in the corresponding carousel location.

Per Machine

This parameter only needs to be defined per machine and so is shared between materials (unlike other cutting data parameters which are defined per machine per material).

Material / Machine Management

The cutting parameters / feeds & speeds section of the tool properties is defined for the active machine / material. This allows you to setup your tools with different values for each material or machine and switch between easily depending on the material you're going to use for the current job.

Material

The combo box is used to change active material. This can also be done by going to the Material Management dialog where materials can be added, removed or edited.

Machine

The combo box is used to change active machine. This can also be done by going to the Machine Management dialog where machines can be added, removed or edited.

Online Tool Database

The tool database can be stored and linked to your portal account so that it can be retrieved at any point from a different installation. For this, the software needs to be logged in to the portal account. Then, the database can be uploaded / download on request.

Login

Login to the portal to be able to access the currently stored tool database and / or upload your existing local one.

Download

Download the tool database stored on your portal account to replace your existing local tool database. This can be used for when we know there is a more up-to-date version online. 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.

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:

test
Round-over
test
Ogee
test
Profile Cutting Strategy with Form cutter

Custom Form Cutters

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

Geometry

Only draw the Right-hand side of the cutter geometry to the correct size and scale as shown in the image above. The shape can be a combination of Lines, Arcs and Bezier spans.

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

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

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

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 Aspire 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.

test
Burn Rate 50
test
Burn Rate 100
test
Burn Rate 200

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

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

Example

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

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

+ Commands output when the jet is turned on

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

begin JET_TOOL_ON

"M4[P]"

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

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

+ Commands output when the jet is turned off

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

begin JET_TOOL_OFF

"M5"

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

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

+ Commands output when the jet power is changed

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

begin JET_TOOL_POWER

"[P]"

Modify Existing Blocks

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

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

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

Example

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

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

+ Commands output for feed rate moves

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

begin FEED_MOVE

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

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

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

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

+ Command output after the header to switch spindle on

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

begin SPINDLE_ON

"[S]M3"

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

+ Commands output for the plunge move

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

begin PLUNGE_MOVE

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

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

Explicitly Mark the Post Processor as Laser Capable

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

Example

LASER_SUPPORT = "YES"

SketchUp Files

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

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

Exploded Flat Layout

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

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

Part Orientation

This section controls what 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 Aspirecan 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, Aspire offers the option to refit circles and arcs to imported data.

test
Options Checked ✓
test
Options Unchecked

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

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

Data to Import

A SketchUp model will often contain parts that you do not wish to machine (such as hinges, knobs etc.) or data which will be cut from different thicknesses of material and hence different parts need to be imported into different Aspire 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 Aspire. 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, Aspire 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 Aspire. 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 Aspire 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 Aspire 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'. Aspire 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 Aspire 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.

test
Moulding Toolpath - Create Sharp Corners Un-Checked
test
Moulding Toolpath - Create Sharp Corners Checked ✓

Boundary Offset

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


Use automatic boundary offset

When this option is selected, Aspire 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.

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.

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.

Modelling 3D Rotary Projects

Elaborating 2D designs with 3D clipart pieces

This section will present how to add 3D clipart to basic fluted column presented in Simple rotary modelling using 2D toolpaths.

A simple way to start with 3D rotary models is to use add pieces of decorative clipart that is provided with Aspire. This process is very similar to adding clipart to single - or double - sided project, however there are some additional considerations that are specific to wrapped rotary machining.

To start, switch to the Clipart tab. Then choose a piece of clipart and drag and drop it into the workspace. Aspire will show following message:

To understand this message, we need to consider the flat view of our model, after importing the clipart. Flat view can be accessed by clicking Auto Wrapping button.

test

As can be seen, the model contains only the selected decorative piece on the flat plane. Although the column is obviously a cylindrical solid, so far we only used 2D toolpaths to carve details on the surface of cylinder. So the fact that machined piece is a cylindrical solid, derives only from fact that the blank is a cylindrical solid itself. Aspire allows the 3D model to also describe a solid body.

In this example the intent is to only place a decorative piece on the surface, rather than define body of the column. Aspire can see that we did not model a body and we are placing a piece of clipart, that is likely to be placed at the surface. By responding 'Yes' to the message we can confirm that it is our intent to use the component to decorate a surface.

Note

The above message is only displayed when the 3D model is empty. Regardless of user choice, this message will not be displayed again for this project.

More clipart can be placed as desired. Then the 3D view can be inspected. Once design is finished it is time to create toolpaths. In order to create 3D roughing toolpath, use the 3D Roughing Toolpath. Then create 3D finishing toolpath, using 3D Finish Toolpath. Select settings that are most appropriate for given application, while remembering which axis is rotating. The choice of axis may be particularly important if rotation axis speed is slower than linear axis.

In this example the decorative clipart that was added was not recessed. That means that after 3D machining the flat areas around clipart will be recessed due to clipart 'standing out' of the flat surface. Therefore existing 2D toolpaths needs to be projected. This can be accomplished by selecting Project toolpath onto 3D model option and recalculating the toolpaths.

Making a tapered column

This section will explain how to make a tapered column by modifying the basic design from previous section.

So far only the surface details were modelled. In order to make a tapered shape, we need to model 'body' of the shape in addition to surface details. For that purpose, zero plane component can be used. It is added automatically for rotary jobs.

Double-click the zero plane component to open Component Properties. Enter 0.8 in the Base Height box. Select Tilt option. Click Set button in Tilt section, then switch to 2D view and then click in the middle left and then in the middle right. Set the angle to 3 degrees.

Since the modelling plane was adjusted for placing component on the surface, it needs to be adjusted again, so the component body is not 'inflated'. To do that open the Material Setup form. Adjust modelling plane by moving the slider down, until the Gap Inside Model is 0.

After modelling a tapered shape, the 3D model of column will have a desired shape. However clipart pieces in the narrower parts have been distorted, as can be seen below. To fix that, one needs to stretch the components in the wrapped dimension, to compensate for distortion.

test
Tapered column with distorted clipart
test
Tapered column with clipart stretched to overcome distortion

The distortion that has been demonstrated above, applies also to toolpaths. That means that wrapped toolpaths will match flat toolpaths only at the surface of the blank. The closer to the rotation axis (i.e. deeper) the toolpath is, the more it will be 'compressed'. This fact have a profound implication for 3D toolpaths. Consider the example shown below.

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

Modelling turned shapes

This section will present a basic technique for creating turned shapes.

Modelling turned shapes is quite easy. It requires a vector representing a profile of the desired shape and a Two Rail Sweep tool.

To start, create a new rotary job. Then either draw a profile using available drawing tools or import profile vector. This example used a chess pawn profile, as can be seen below.

Open the Two Rail Sweep tool. When the rotary job is created, the software inserts a special layer called '2Rail Sweep Rails'. It contains two blue lines on the sides of the job, that are perpendicular to the rotation axis.

Select both of those rails and click the Use Selection button. The rails will then be highlighted. Then select the profile vector and click apply. Inspect the 3D view to verify the results.

Modelling cross section

This section will explain how to model desired shape using Vector Unwrapper.

The Vector Unwrapper is useful when rather than modelling a profile along the rotation axis, it is more intuitive to specify a desired cross section. The tool transforms a vector, representing a cross section, into a profile vector that can be subsequently used with Two Rail Sweep tool.

Suppose we would like to create a hexagonal-shaped column. Let's start by creating a new rotary job. In this example job has a diameter of 6 inches and is 20 inches long. X axis is the rotation axis and Z origin has been placed on the cylinder axis.

We need to create a hexagon using Draw Polygon tool. This vector will serve as a cross section and can be placed anywhere in the 2D view. In this example the material block diameter is 6 inches, so the radius of the shape cannot exceed 3 inches.

When the shape is created, select it and open Vector Unwrapper. The tool will display a crosshair in place where the rotation axis is crossing the profile and a circle with the diameter of the material block. This will help you determine whether the shape with such cross profile will fit in current material block.

In this example, the Use Center of contour option was used. That means that rotation axis will be placed in the centre of vector's bounding box. One can also tick Simplify unwrapped vectors option to fit bezier curves, instead of using series of very short line segments. After apply is pressed, the unwrapped version of the selected cross section will be created, as have been shown below.

This example shows the unwrapped vector for a cylinder rotating around the X axis. If your rotary axis is aligned along Y the unwrapped vector will be horizontal. It is worth noting that unwrapped profile have 'legs' on each end. Those are needed to ensure that correct height will be used in the next step.

The tool automatically creates layer called 'Unwrapped Vectors Drive Rails' on which it places two blue line vectors on job sides, parallel to the rotation axis. In order to extrude the profile, open the Two Rail Sweep tool. Then select top and then bottom rail (left and right when Y axis is rotation axis) and confirm selection by clicking Use Selection button. The rails will now be highlighted. Now click on unwrapped vector and press apply. The 3D view will show a hexagonal column, that can be seen at the beginning of this section.

Modeling Plane

The desired cross-section will only be achieved if modelling plane is positioned in cylinder centre. That means that Gap Inside Model is reported as 0 in Material Setup form. Otherwise the resulting model will have incorrect diameter and the cross section will become rounded.

The Vector unwrapper is not restricted to simple shapes. In principle it is always possible to use convex shapes and certain concave shapes. The example below shows a heart profile unwrapped.

test
Heart-shaped vector and its unwrapped version
test
Extruded heart shape

If cross section in question is concave, one could imagine straight line starting in the center of the shape and touching a point on the boundary. If the second points keeps travelling along the boundary and each line is not crossing another point on the boundary, then it is possible to use this cross section. If the line does cross more than one point on the boundary, this part of the cross section will not be represented correctly.

All the examples so far used a single cross section. However it is also possible to use multiple cross sections.

Let's take another cross section and open Vector Unwrapper. Then drag the rotation axis handle a bit down from the center. If snapping is enabled, it can be used to help position the rotation center, as can be seen below.

Once we have another unwrapped cross section, it is possible to use both during Two Rail Sweep. For example unwrapped heart profile can be placed twice on the left and twice on the right. The second unwrapped profile can be placed twice in the middle. Such arrangement may result in shape morphing, as can be seen below.

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:

test
Bend Text Upwards
test
Bend Text Downwards

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

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

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

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

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.

test
Rotate Copies selected
test
Rotate Copies not selected

Angle

Total Angle

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

Step Angle

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

Note

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

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

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

Preview All Sides

This option animates all calculated toolpaths cutting into the material on both sides if working in a two sided environment without being in the 'Multi Sided View' mode (This option will be grayed out if working in a single sided setup)

Preview All Toolpaths


This option animates all calculated toolpaths cutting into the material


Preview Visible Toolpaths

Previews all the visible toolpaths

Reset Preview

Resets the material back to a solid block

Save Preview Image

Saves an image of the 3D window as a BMP, PNG, JPG or GIF file

Turn and Spin

The Turn and Spin tool allows you to create a 3D component by turning or spinning a cross section (an open vector)

Turn

Turn takes a profile and turns (rotates) it around line from start point to end point to create a rounded symmetrical shape. To turn a shape select the vector cross section you want to turn and use the Turn (Rotate) option, this cross section should represent the silhouette of the shape you wish to create. You can click to create your 3D turned shape.

The profile to be turned can run beneath the line between the two end points

Spin

Spin takes a profile and spins it around the left end point of the cross section to create a circular component based on the profile shape of your cross section. To spin a shape select the vector cross section you want to spin around the left end point and click to create your 3D spun shape.

Note

The Spin Tool will always Spin around the left end point, which may require you to move your vector to the right side of your job to accommodate the vector being spun to create the spun shape.

Scale to Exact Height

Checking ✓ this option scales the shape calculated so its maximum height is the value entered in the Height area of the form.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Nest Parts

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

Object Selection

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

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

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

Tool and Clearance Settings

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

Tool Dia. (D)

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

Clearance (C)

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

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

Border Gap

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

test
No Border Gap
test
Border Gap

Part Nesting Options

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

Rotate Parts to find best fit

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

test
Rotate Parts Enabled
test
Rotate Parts Disabled

Mirror parts to find best fit

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

Allow parts inside other parts

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

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

test
Original
test
Parts Nested inside other parts

Nest two-sided parts

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

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

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

test
Double-sided part before selection
test
Double-sided part when selected

Remove original parts

If this option is checked the original parts are removed in the nesting rather than duplicated in the nest.

Sheet Options

Nest From

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

Nest Direction

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

test
Along X
test
Along Y

Individual Part Properties

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

Nest boundary

A nesting boundary can be specified by choosing a layer whose vectors will represent the nesting boundary. Multiple vectors can be used. The nesting process will try to place the nested objects inside the vectors of the boundary layer.

Active Sheet

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

Nesting Sheets

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

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

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.

test
test

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
test
Double click to add slice

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

You can also manuipulate the slices within the 3D View

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

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.

test
Loose
test
Tight

Noise Filter

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

Bitmap Fading

Preview

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

Apply

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

How to Get Started

The first stage in any project is to create a new blank part or import some existing data to work with. At this stage a number of parameters need to be defined relating to the size of the part and its position relative to the datum location on the CNC machine. Later, once the part has been defined and you have started working, you may want to change the size of the material, import additional data and generally manage the project operation. In this section of the manual the initial creation of a part will be covered along with all the icons which appear under the File Operations section of the Drawing Tab.

When you first start the program you will see the Startup Task options on the left hand tab and also a list of your 4 most recently opened Aspire parts (this is a rolling list that will be populated each time you run the software and may initially be empty).


Startup Tasks and Recently Opened Files

When you first start the program you will see the Startup Task options on the left hand tab and also a list of your most recently opened Aspire parts.

The first choice is whether you want to Create a new file or Open an existing one. 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.

The size forms may be limited

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).

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:

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

Setting up a rotary project

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

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

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

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

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

Importing the file and orientating it

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

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

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

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.

test
test
The same model imported without distortion

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

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

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.

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

Scaling imported model

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

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

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,

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

Project Saving

If you're working on a job and the software crashes, the first thing it will try to do is to save your project. The project will be saved alongside your original to avoid accidentally corrupting your original file.

Report the crash

A dialog will pop up asking you to upload the crash information which will help us track down the issue. Any information you can think of would be greatly appreciated and will help us fix the issue in a timely manner.

Description

Please try to remember what you were doing at the time, and describe it for us. Please include any information you can think of. Any bit of information can help us track the issue quicker, so we greatly appreciate that.

Information

You can include your name and e-mail to allow us to get back to you with questions in case we need more information. For example, we may need the project that you were working on. This data will not be used for any purpose other than to help us track down the issue.

Internet

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

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

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:

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

Horizontal Stretch

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

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

Edit Text

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

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

test
Rectangular Border
test
Oval Border

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

test
Rectangular Border
test
Oval Border

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 Aspire.

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 Aspire 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 Aspire...

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

test

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 Aspire 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 Aspire to retrieve your license details automatically.

At this point Aspireshould 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 Aspire will automatically be restarted to apply the license changes. If you do not select this option the license changes take effect the next time Aspire 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,

  1. Loading from a File
  2. 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

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

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.

Create Component from Bitmap

This tool lets you automatically create a 3D Component from a Bitmap.

If no Bitmap is selected in the 2D View, then a File dialog will open allowing you to select an image file from one of the drives on your computer. This method of component creation bypasses the need to convert the image when importing which potentially reduces the number of color shades, so this second method is the best way to directly convert Bitmap files to components in Aspire.

The Component from a Bitmap is automatically scaled and set to Add to other Components by the software so will typically need to be edited using the Component Properties icon to adjust height or Combine Mode and the Transform tools to adjust its size and position.

Converting selected bitmap

If you have a selected Bitmap in the 2D View this will automatically create a new component derived from that Bitmap, the Component will have the same name as the original image.

Converting without bitmap selected

If no Bitmap is selected in the 2D View, then a File dialog will open allowing you to select an image file from one of the drives on your computer. This method of component creation bypasses the need to convert the image when importing which potentially reduces the number of color shades, so this second method is the best way to directly convert Bitmap files to components in Aspire. This is especially important for 16-bit images.

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).

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.

test
3D Tab

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

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

test
How the lenght and thickness change the tab size

Profile Options

The Profiling options section of the toolpath form contains five additional pages, each of which allows a particular set of Profile machining options to be specified. The precise number of option pages will depend on which Toolpath strategy you are currently using. The full range of option pages are:

  • Ramps
  • Leads
  • Order
  • Start At
  • Corners

These help control ways to ensure the parts are held in place and machined as easily as possible while ensuring the highest quality edge finish.

Each set of options can be accessed by the tabs at the top of the Profile options section.

Ramp

Ramp moves are used to prevent the cutter from plunging vertically into the material. The cutter gradually cuts at an angle dropping into the material significantly reducing cutter wear, heat build-up and also the load on the router spindle and Z axis of the machine. If multiple passes are required due to the Pass Depth being less than the Cut Depth, the ramp moves are applied at the start of each level. All ramp moves are performed at the plunge rate selected for the current tool.

Smooth

This option creates a smooth ramp into the material using either the specified Distance or Angle.

When a Lead In distance has been specified, the option Ramp on Lead In disables the distance and angle options and automatically limits the ramp moves to only be on the lead in portion of the toolpath.

Zig Zag

This option ramps into the material by Zig-Zag backwards and forwards using either the specified Distance or Angle and Distance.

The Distance option ramps into the material, zigging for the specified distance in one direction then zagging back over the same distance.

The Angle option is typically used for cutters that cannot plunge vertically but have an entry angle specified by the manufacturer.

Spiral

Checking ✓ this creates a continual spiral ramp, these are only available when the toolpath does not include lead in moves.

This option ramps into the material over the complete circumference of the profile pass. The angle is automatically calculated to ramp from the start point to full depth over the perimeter distance around the job.

The rate at which the cutter ramps into the material is determined by the Pass Depth specified for the cutter. For example, Spiral Profiling 0.5 inch deep with a cutter that has a Pass depth of 0.5 or greater will spiral down in 1 pass. Editing the Pass depth to be 0.25 inch results in the 2 spiral passes around the profile.

Leads

Lead in / out moves can be added to profile toolpaths to help preventing marking the edges of components with dwell marks that are typically created when a cutter is plunged vertically on the edge of the job.

Straight Line Lead

This option creates a linear lead onto the cutter path using the Angle and Lead length distance specified.

The toolpath will lead onto the selected edge at the specified Angle.

Checking ✓ the Do lead out option results in an exit lead being added at the end of the toolpath off the machined edge.

The Overcut Distance forces the cutter to machine past the start point and is often used to help produce a better edge quality on parts.

Circular Lead

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

The toolpath will curve onto the selected edge, tangent to the direction of the vector at the point it reaches the actual geometry edge.

Checking ✓ the Do lead out option results in an exit lead being added at the end of the toolpath off the machined edge.

The Overcut Distance forces the cutter to machine past the start point and is often used to help produce a better edge quality on parts.

Order

The order tab allows you to specify the approaches the program will use to determine the best order to cut your vectors. You can specify multiple options, in which case the program will calculate the result of using each option and select the one which results in the shortest machining time.

Vector Selection Order

This option will machine the vectors in the order in which you selected them. If you have vectors inside each other (like in the letter 'O'), the inner vector will always be machined before the outer one regardless of the selection order.

Left to Right

This option will join up parts on the left of the material first and move across to the right.

Bottom to Top

This option will join up parts on the bottom of the material first and move up to the top.

Grid

This option will join 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.

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

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.

test
Chamfer Outside & Down. With pocket clearance outside
test
Chamfer Outside and Up. Clearance pocket inside the 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.

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

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.

Load Toolpath Template

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

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

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

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

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 Aspire has a Layer function for managing 2D data. The Layers are a way of associating different 2D entities together to allow the user to manage them more effectively. Layers will be described in detail later in the relevant section of this manual. If you are working with a 2 Sided project you can switch between the 'Top' and 'Bottom' sides in the same session, enabling you to create and edit data on each side, and using the 'Multi Sided View' option you can view the vectors on the opposite side. 2 Sided Setup will be described in detail later in the relevant section of this manual.

Vectors

Vectors are lines, arcs and curves which can be as simple as a straight line or can make up complex 2D designs. They have many uses in Aspire, such as describing a shape for a toolpath to follow or creating designs. Aspire contains a number of vector creation and editing tools which are covered in this manual.

As well as creating vectors within the software many users will also import vectors from other design software such as Corel Draw or AutoCAD. Aspire supports the following vector formats for import: *.dxf, *.eps, *.ai, *.pdf, *skp and *svg. Once imported, the data can be edited and combined using the Vector Editing tools within the software.

Bitmaps

Although bitmap is a standard computer term for a pixel based image (such as a photo) in *.bmp, *.jpg, *.gif, *.tif, *.png and *.jpeg. These file types are images made up of tiny squares (pixels) which represent a scanned picture, digital photo or perhaps an image taken from the internet.

To make 3D models simple to create, Aspire uses a method which lets the user break the design down into manageable pieces called Components. In the 2D View a Component is shown as a Grayscale shape, this can be selected and edited to move its position, change its size etc. Working with the Grayscale's will be covered in detail later in this manual. As with bitmaps, many of the vector editing tools will also work on a selected Component Grayscale.

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

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.

test
Toolpath for coves of the column
test
Toolpath for flutes of the column

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.

test
Cut-out toolpaths in 2D view
test
Finished part after adding cut-out toolpaths

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

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.

test
Vectors used to create spiral flutes
test
Spiral toolpaths in flat view

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

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

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

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

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

Smart Snapping

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

Note

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

Note

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

Snapping lines can be drawn from:

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

Note

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

Cursor

Type

Description

Object Bounds

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

test
test

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.

test
test

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.

test
Bounding Box
test
Object Center

Vertical and Horizontal Lines

Nodes

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

Vectors

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

test
Vertical
test
Horizontal

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

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

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.

test
test

3D Segmenting

The Segment tool can be used to split a 3D model into separate chunks or segments to allow them to be machined using a 3-axis CNC machine.

To get to the segmenting tool you first have to import a 3D model using the standard Model Import Dialog.

There are 4 main sets of options:

  • The mode selection controls which mode we are in.
  • The Segmenting Plane section controls the placement of the next segmenting plane. This is mostly for setting exact values. Most of the time, the 3D view controls are more convenient.
  • The Segments Viewer gives an overview of the segmenting tree. This shows all of the segments and how they are related to one another.
  • The Import Options can be used to control the settings used when we are ready to import the segmented model into the job.

Usage Overview

The segmenting tool works by incrementally splitting the imported model into blocks. The segmenting plane is placed in the model, and we press . Each segmenting operation produces two new segments, one for above the segmenting plane and one for below.

test
Model before segmenting
test
Segment above plane
test
Segment below plane

The Segments Viewer shows that this segmenting operation has produced two new segments. Each segment can be selected by clicking in the tree.

test
Result after segmenting once

Once a segment has been selected it forms the base for future segmenting operations, and this segment can be further divided, into more segments. The tree reflects the fact that one of original segments has been chosen, and the tree and the parts in the 3D view are coloured to show the result.

test
Further segmenting a segment.
test
test
Segmenting a segment produces two new parts. Each is colour coded

At each step the orientation and position of the segmenting plane can be adjusted to ensure that the resulting segments are appropriate for machining. To adjust the plane you can use one of the dynamic handles shown in the 3D view.

Once the model has been segmented enough then we can enter layout mode. Within layout mode we can see the segments created and how they will look once imported into the job.

test
Layout Mode

At this stage each of the segments can be flipped to a desirable orientation. This is done by selecting a segment and cycling through the different possible orientations using the arrow buttons in the segment positioning section.

test
Original orientation in layout mode
test
Correct orientation

If it is desired to position the segment at an orientation which is not present in the provided cycle-through options, then the segment can be interactively rotated. Select the segment in question and press the shortcut on the keyboard. This will display a dynamic rotation handle centred on the selected segment which can be used to interactively orient it. Once you are happy with the positioning, press the keyboard shortcut once again to hide the rotation handle.

The other key feature of the layout mode is the visualize undercuts option. When this option is checked then undercut areas (which cannot be cut with a regular 3-axis CNC machine and so are ignored on import) are highlighted. If these areas are significant then it may be desirable to return to the edit mode and segment in a different way to remove these undercut areas.

test
Undercuts shown in pink

With the dynamic nature of this tool we strongly recommend the viewing of the corresponding video tutorial for a more through coverage of the features

Note

If at any point errors occur with importing or undercut analysis then this might be caused by importing 3D models which have self-intersections. The segmenting tool cannot be used on such models.

Mode Selection

The mode selection switches the tool between layout and edit mode:

  • In Edit mode the model can be segmented into different sized segments.
  • In Layout mode the segments defined in edit mode can be rearranged, reoriented and visualized.

Segmenting Plane

The segmenting plane section controls the positioning of the next segmenting plane. This plane can be positioned using the 3D view controls, or by adjusting the numerical values in the edit boxes. Once a desired position and orientation have been chosen then pressing the button will produce a new segment.

Segments Viewer

The segments viewer section shows all of the segments in tree view. The root of this tree is the original model. Whenever a segmenting operation occurs then the current segment in the tree gets two children, these two children represent the resulting two segments produced when slicing along the segmenting plane.

At any point any of the segments in the tree can be selected. The 3D view will show only this segment. If this segment has been further segmented then those segments will be displayed visually by having different colours in the 3D view.

Undoing a segment

At any point any segmenting operation can be undone. To undo, select a segment from the tree, right-click and choose Delete children. This will remove the children from the tree and join the corresponding segments back together again.

Note

You can delete the children of any segment, this operation is not restricted to just the most-recently created segments. If at any point you want to restart segmenting altogether you can just delete the children of the top-level node.

Rearranging Segments

You can drag and drop segments on top of one another in the tree to merge two segments together. The resulting segment will just be the result of combining two segments. This can be useful for both recombining or rethinking a segmenting approach. It is also useful if you want to create a segment for a particular part, but that segment includes other parts you don't want.

test
Want to create a segment of the face without the bottom stand
test
Remove the lower stand with another segmentation
test
Rejoin the base with previous segment

Import Options

Create Backface Caps

If this option is selected then the back of any segment is closed off with a plane. This option may be desireable in mold creation.

Resize Material To Fit Slices

If this option is selected then the job size will be adjusted to accomodate the newly created segments.

Create boundary vectors

If this option is checked boundary vectors are created for the top and bottom boundaries of the segments.

Re-importing a segmented model

Once the segmented model has been imported it may be re-imported by right - clicking any of the imported segments in the component tree and selecting Re-import model. This will return the model to the last known state in the segmenting tool before import.

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

test
Add
test
Subtract
test
Merge
test
Low
test
Group

Grouping

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

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

Selection

Components can be selected in 3 ways:

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

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

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

Selection in the Component Tree

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

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

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

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

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

Selection in the 2D View

The 2D component previews behave exactly the same way as vectors or bitmaps. They can be selected by a single, left-click. Several component previews can also be 'shift selected' (see above). Clicking on selected component previews again activates their interactive transform handles. These can be used to move, rotate or stretch the 2D component preview and its associated 3D component.

Selection in the 3D View

Because the left mouse button is used for twiddling the 3D view itself, a single left-click cannot be used for component selection directly. However, Aspire'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 Aspire 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.

Create Rounding Toolpath

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

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

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

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

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

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

Blank Size and Shape

The gadget supports creating a toolpath to machine either a square blank or a round one. In this section you specify the shape of your initial blank and its dimensions. The diagrams show which dimensions are being specified.

Machining Method

The gadget offers a choice of three types of machining and for all types you can enter an allowance that will be left on the final shape if required. The Radial and Raster options can be used with either square or round blanks, the Optimized Raster can only be used for square blanks.

Radial (around cylinder)

This option creates a toolpath which rotates the blank around its axis 360° before stepping over to the next pass by the tool stepover distance and rotating the blank back again.

Raster (along cylinder)

This option machines along the length of the cylinder before incrementing the rotary axis round by an amount equal to the tool stepover and then returning the tool back along the cylinder axis. For many machines where the rotary axis is often slower than the X or Y axis, this strategy may allow shorter machining times.

Optimized Raster (along cylinder)

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

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

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

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

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 Aspire'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

  1. The Main Menu Bar (the Drop Down Menus) along the top of the screen (File, Edit, Model, Toolpaths, View, Gadgets, Help) provides access to most of the commands available in the software, grouped by function. Click on any of the choices to show a Drop-Down list of the available commands.
  2. The Design Panel is on the left side of the screen. This is where the design tabs can be accessed and the icons within the tabs to create a design.
  3. The Toolpath Tab is on the right side of the screen. The Top section of the toolpaths tab houses all of the icons to create, edit and preview toolpaths. The bottom half shows you toolpaths that you have already created.
  4. The 2D Design window is where the design is drawn, edited and selected ready for machining. Designs can be imported or created directly in the software. This occupies the same area as the 3D View and the display can be toggled between the two using F2 and F3 or the tabs at the top of the window.
  5. The 3D View is where the composite model, toolpaths and the toolpath preview are displayed.
  6. If you wish to see the 2D and 3D views simultaneously, or you wish to switch your focus to the Toolpaths tab at a later stage of your design process, you can use the interface layout buttons (accessible in the 2D View Control section on the Drawing Tab) to toggle between the different preset interface layouts.

Managing the Interface

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

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

Accessing Auto-hidden tabs

If a tools page is auto-hidden (because it is currently unpinned, see pinning and unpinning tools pages, below), then it will only appear as a tab at the side of your screen. Move your mouse over these tabs to show the page temporarily. Once you have selected a tool from the page, it will automatically hide itself again.

Pinning and unpinning tools pages

The auto-hide behavior of each tools page can be controlled using the push-pin icons at the top right of the title area of each page.

Default layout for Design and Toolpaths

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

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

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.

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

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:

test
Single Point tools have a single point for cutting a single thread at a time
test
Multi-Point tools have multiple cutting teeth. They will cut all the threads with a single rotation

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.

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.

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.

Gadgets

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

Install New Gadget...

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

Gadget Shortcuts

Opens Gadget Shortcuts dialog.

Installing Gadgets

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

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

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

Note

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

Running Gadgets

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

Alternatively Gagdets can be assigned shortcuts.

Gadget Shortcuts

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

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

Preinstalled Gadgets

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

Wrapping Sub-menu:

Note

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

Developing Gadgets

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

Please Note

This will require knowledge of programming.

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

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

Offset Model

I am only for

The Offset model tool creates a 3D offset of the composite model.

To use the tool, specify the distance that you want to offset the model.

Click on the button to see the results of the offsetting.

Click to proceed or click to exit the form.

The Clip Z values to the Zero Plane option will ensure that the final result will always be positive. When used on models with areas that end up lower than the zero plane these parts of the model will be removed leaving only the positive values. This can be helpful when you have a flat plane as part of the model to avoid it being effectively lowered by the offset amount.

Using this function you can offset with either positive or negative values.

test
Original model
test
Negative Offset
test
Positive Offset

Note

Clicking the Preview button repeatedly will apply your chosen offset multiple times. Click the Cancel button to remove all effects of the previews.

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.

Keyhole Toolpath

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

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

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

The data to be entered falls into three separate categories.

Slot Parameters

In this section of the form you specify the direction the slots will be machined and also the depth and the length for the slots.

Preview Drawing

To help with visualisation of the slot, the gadget can draw a vector outline of how the slot will appear on the surface of your job. This drawing is optional and if you un-check the Create Preview Vectors for outline on surface check box you do not need to fill in the parameters in this section. If you do want previews drawn, you can specify the entry hole diameter which will be created by your keyhole cutter and also the diameter of the slot the tool will create on the surface. You can also specify the name of the layer the vectors will be created on.

Toolpath Parameters

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

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

Right Mouse Click Menu

Clicking the ►RIGHT hand mouse button in different places in Aspire 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: to convert the span to a Line, Bezier (curve) or Arc, Insert a Point, Cut the Vector at that point, Delete the Span, or Insert a Midpoint. Keep Bezier Tangency, which will fix the start and end directions of Bezier curves when they are being dragged directly, can be toggled on or off. From this menu you can also Reverse the direction of the selected vectors, Close any selected open vectors, Join two selected open vectors or Exit node editing mode. Many of these have corresponding Shortcut keys (shown to the right of the command in the menu) which can be selected from the keyboard when the mouse is in position (over a node-edit vector span) instead of Right Clicking the mouse button to access the menu.

Node Editing Menu

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

Bitmap Properties Dialog

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

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.

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

Offsetting Open Vectors

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


Advanced Modelling of 3D Rotary Projects

Modelling 3D spiral features

In this section we will show how to use level-wrapping feature to wrap a design in spiral manner around a column.

The workflow for creating spiral toolpaths has been presented in the Simple rotary modelling using 2D toolpaths chapter. The basic idea involved creating a line at a proper angle to the rotation axis, that exceeded the 2D boundaries. When 2D toolpath is created based on such a line, it will be wrapped around material cylinder, creating a spiral.

This guide will build on that basic idea. The task is to create a horizontal strip with desired pattern and then wrap it like a ribbon around the cylinder.

To help with that task, it is important to create some helpful vectors first. We need to create lines, that will become boundaries of our strip. In this example the strip was being wrapped four times around full length of material. This example assumes that rotation axis is parallel to X axis.

To start, select Draw Line/Polyline tool and draw a horizontal line at the bottom of the job from left to right. If it is desired for the spiral pattern to only fill part of the cylinder length, this horizontal line should be drawn only in th desired location. While the drawing tool is still active, type 90 into Angle box and type y * 4 into Length box and pressing =. We used y * 4 formula so the strip will wrap 4 times. Then press Add button to add a vertical segment.

Now, start a new line that connects the horizontal and vertical lines, forming a triangle. Once this line is created, horizontal and vertical lines can be removed.

The line that we just created will form a bottom of the strip. Now copy this line and place line so its bottom left end coincides with top left corner of the 2D job. This line will form a top of the strip. Then make another copy and place it in the middle. This middle line will be used later to position our design within strip. All three lines have been shown below.

test
test

Next step is to find out the required length and width of the strip. We will need a few extra vectors to accomplish that.

Let's copy one of the created three lines and rotate by 90 degrees, to get a line that is perpendicular to the strip. Then place it in such way so it crosses the strip. This will help us measure the width.

Then copy the perpendicular line and place it so it touches the top line. Then extend the bottom line, until it crosses the perpendicular line we just added. This will help us measure the length of the strip.

The easiest way to achieve that, is to create a textured component. To do that, select the design in the component tree and activate the Create Texture Area tool. This example used the default settings of the tool. The tool will create a new component that will fill the whole 2D job boundaries. The component itself will be filled with the design in tiled manner. Now use the Set Size tool to resize textured component to match the strip size.

Now the component have to be rotated and moved to fit between the lines you have drawn at the beginning. This process can be made easier by utilizing Copy Along Vectors tool. To proceed, activate the tool and select the textured component first, then select the middle line in the strip while holding Shift. Make sure that Align objects to curve option is selected and use Number of copies option. Since our strip has already have a correct size, we only need one copy. However the tool would place the middle of our component at the beginning of the line only. If you enter 3 as the number of copies, then the tool will place two copies of component at each end and in the middle. Afterwards the copies at the ends can be simply deleted. The picture below shows the strip in the 3D view after being correctly positioned.

test
test

As can be seen, the strip disappears as soon as it leaves the material boundaries. In order to make it wrap around, we need to create a new level in the component tree and move the texture component into it. Then right click on the newly created level and right click. From the pop-up menu select wrapping. After that wrapping will occur.

Note:

Wrapping can be enabled on any level in component tree and combined with mirror mode. If the level wraps on itself, then intersecting areas will be merged regardless of level's combine mode. If it is desired to create e.g. a woven pattern, then place left-hand spiralled component and right-hand spiralled components in different separate levels, both with wrapping enabled.

The last step is to make column endings. For that purpose the third level was created, with Combine Mode set to Merge. This way the spiral pattern will be 'hidden' at the ends. A circular 3D tab clipart was placed at each end, and stretch vertically to match the job boundaries.


Modelling twisted shapes

This section will show how to create twisted shapes, using a combination of level-wrapping and Vector Unwrapper tool.

In this example a new rotary job was created, with a diameter of 6 inches and length of 20 inches, rotating around X axis. To start, we need a cross-section vector. In this example a 5-armed star was used. To create a star, we can use Draw Star tool. This example used Outer Radius of 3 inches, to match the radius of the material.

The next step is to unwrap the cross section. In the case of the star however, the center is not the same as center of star's bounding box. To find the real center, one can draw a line from two of the star corners. Then open Vector Unwrapper and select the star. Then drag rotation center and snap it to the intersection of the lines, as can be seen below.

test
Using Vector Unwrapper with the star-shaped vector
test
Rails and uwrapped star


Once the star is unwrapped, we need to create rails, that will make spiral when wrapped. To do that, select Draw Line/Polyline tool and draw a horizontal line at the bottom of the job from left to right. While the drawing tool is still active, type 90 into Angle box and type y * 2 into Length box and pressing =. We used y * 2 formula so the star will make 2 revolutions Then press button to add a vertical segment. Finally, start a new line that connects the horizontal and vertical lines, forming a triangle. Once this line is created, our horizontal and vertical lines can be removed.

Next step is to copy the line and place it so its bottom left end coincides with top left corner of 2D job.

Once the the rails are ready, one could use a Two Rails Sweep tool. However, since rails exceeds the 2D job boundaries, the created sweep will be cropped as soon as those boundaries are exceeded.

To overcome that, select both rails, open Draw Rectangle tool and press . This will create a bounding box containing the rails. Now, write done the size of the box and save current project. Then create a new single-sided project with the slightly bigger than the bounding box. Use the Import Vectors option from the main menu and select the previously saved file. Now select the rails and press F9 to center them.

Now use Two Rail Sweep tool. When component is ready, save the file.

Now re-open the original rotary project. Use Import Component and select the single-sided project created in the step above. Move the component to the desired location. Then, create a new level, move the component there and enable wrapping.

Using single-sided modelling tools

This section will present how to use single-sided modelling techniques in rotary projects.

Users familiar with modelling techniques used in single-sided projects may find them more convenient for modelling certain shapes. This example uses two vectors, representing side cross section of the table leg and a few of half cross sections for different parts of the table leg. Those vectors are presented below.

One can simply treat the side cross section as rails and use the Two Rail Sweep tool, placing the half cross sections at appropriate locations. This way half of the leg can be modelled very quickly, with the result that can be seen below (using flat 3D view).

In order to use the created model in a rotary project, we need to export and then import it back. Although it is possible to do this with two sessions of Aspire, it can also be done within a single session with rotary project. To export the leg model, make sure no other components are visible (including the automatically added zero plane) and open the Export Model tool while holding down Shift. Pressing Shift allows to open the export tool in single-sided, rather than rotary mode.

Since half of the leg was modelled, Close with inverted front option can be used. The resulting STL mesh can be seen below.

Once component is exported, it can be re-imported as Full 3D model. The model will have a seam, in the place were two halfs were merged. This can be removed using smoothing function of the Sculpting tool.

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 Aspire

License Registration

If you have recently purchased your machine which came with some licencse details for Aspire (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.

Two Rail Sweep

Two Rail Sweep uses a combination of vectors to define a swept 3D Component. The shape is based on two drive rails which can be open or closed vectors and multiple cross sections which are positioned on the drive rails and have to be created using open vectors.

Drive Rail Selection

The first stage of using this tool is to select the vectors which will represent the Drive Rails. From the 2D View use the mouse to select two open or closed vectors then click the button.

In the 2D view your rail vectors will now be colored red (first selected vector) and green (second selected vectors) and show a square green start node indicating the start point of each rail and arrow markers along its length to show the direction the shape will be swept.

The start point and direction may not be what you intended. To change the direction, right-click with the cursor on the drive rail you want to edit and select from the context sensitive menu, you will now see the arrows on the drive rail change direction.

You can also change the order the rails were selected by clicking on this will swap so the red rail becomes green and green becomes red, doing this will cause the cross-sections to hang in the opposite direction. On a closed vector you can change the start point by placing the cursor over an existing node in the drive-rail vector, right-clicking and selecting or you can right-click anywhere on the vector and select Insert Start Point to create a new node which will become the start point.

The button on the form can be used at any time to empty your current selection. This will delete your current shape and deselect all the drive rails and cross section vectors. This can be used if you do not want to create a Component before you exit the form or if you want to select new vectors in the 2D view to use as the drive rail for your shape.

Cross Section Selection

After you have chosen your drive rails the next step is to select one or more cross-section vectors to sweep along those vectors to form a 3D shape. In order for vectors to be used as valid cross-section shapes, they must be open.

Select a vector that you wish to use as a cross-section in the 2D View by left clicking on it with the mouse.

If you are using just a single cross section then you just need to make sure it is selected and then can proceed with the other settings in the form and calculate your shape. If you want to edit cross section positions or add more than one cross section then you will need to attach them to the drive rails.

Select a vector that you wish to use as a cross-section in the 2D View by left clicking on it with the mouse. Now click on the drive rail to attach the cross-section to that vector.

As you move the mouse over a selected drive rail it will indicate with a check mark ✓ that it is a valid place to add the cross section. Once a cross-section has been successfully attached to your drive rail, the 2D view will show a preview using line markers to indicate how the cross section will be positioned when it is extruded.

Two Cross-Sections are always created when you attach the first cross-section to the drive rail - one across the start nodes of each vector and one across the ends. The intermediate lines along the entire length of the rails indicate how the shape will flow between the defined cross sections. You can click the button to create your 3D swept shape.

Using multiple cross-sections

It is possible to extrude between multiple cross section vectors along a drive rail blending from one vector shape to another.

Adding Cross-Sections

To add a new Cross-Section to an existing extrusion, simply select an open vector in the 2D View that you wish to use as a cross-section. With the vector selected, click on the point along the rail to which you wish it to be attached. A new Cross-Section will be inserted at this point and automatically attached to the second rail. On applying the change, the resulting 3D sweep will blend between all the defined Cross-Sections along the rail.

test
Adding Cross Sections
test
Result From Two Rail Sweep

Note

To help differentiate which cross section is being used at each location the software will indicate a colored node at one end of each cross section and place the same colored node on the preview position. This node also indicates the direction the cross section is being 'hung' across the rails. The same cross section vector can be used in multiple locations along the drive rail.

Connecting Rail Nodes

By default, Aspire sweeps the cross-section along the drive rails connecting points at the same proportional distance along each rail's length. So, for example, the positions halfway or three-quarters of the way along each drive rail will be connected by the cross section in the resulting 3D shape.

As the images above show, when the matching proportional positions along each rail do not match the appropriate features of the shape it can produce undesirable results. In this example the corners of the frame design are at different proportional positions along each rail and so the two-rail sweep does not connect the corners. Instead the cross-section appears stretched around the frame, as it is used to connect other points that do match in their proportional distance along each rail.

To resolve this, the software allows you to force the connection of pairs of points along the drive rails. This can either be done manually by inserting and re-positioning the cross-sections across the corners (see sections below for more information on this), or if both the drive rails have the same number of nodes it can be done automatically after you have added the first cross section by right-clicking on the first cross section preview position and selecting Add To All Rail Nodes. This will add that same cross section to every pair of nodes on each drive rail. When the cross section positions are set up correctly then Aspire will sweep the shape between each cross section location and create clean corners as shown in the images below.

Removing Cross-Sections

To remove a Cross-Section, position the cursor over the cross section and press the RIGHT button on the mouse. Select the option to Delete Cross Section from the menu.

You can remove all the Cross-Sections on the drive rails by positioning the mouse arrow over a part of the curve that does not contain a cross section. This will bring up a different context sensitive menu and you can select the options to Remove All Cross Sections.

Altering Existing Cross-Sections

Existing cross-sections can be re-positioned on the drive rail. To do this click on the nodes at either end of the cross section preview in the 2D View (the ones on the rails), hold the mouse down and drag the node to a new position on the curve, let go of the mouse button to release that end of the cross section in its new position. You should make sure you do not drag a cross section past another existing cross section on the shape. If you need to move cross sections out of their current order then you should remove the existing cross section and insert the same shape at the new position so the shape can be created correctly. Any of your current cross-sections can be replaced by selecting a different open vector, moving the mouse over the end node of the cross section you want to change and clicking on it. The node color indicated on the cross section preview position on the curve will change to indicate which vector is now being used at that point in the shape.

Controlling the Swept Shape

There are check boxes in the form that allow you to Scale cross sections with width, Sweep between spans, and Fill center of inner closed vector rails. The Smooth option under the right-click menu allows you to control different aspects of the shape you create with the selected set of vectors.

Scale cross sections with width

As the cross sections are extruded along the rails the user can either choose to retain the exact shape and height of the cross sections or for a more natural look the Scale cross sections with width option can be checked ✓. This will alter the height of the cross section in proportion to the distance between the rails. This means that as the rails get further apart the shape gets higher and as they get closer together the shape gets lower. The image below left shows the result if this option is un-checked and below right with it checked ✓.

test
Scale cross section with width un-checked
test
Scale cross section with width checked ✓

Sweep between spans

This option only becomes active if all selected cross section vectors have the same number of spans and nodes. When checked ✓ it will ensure that as the shape is extruded that it goes from a particular node/span in one cross section to the same node/span on the next cross section. In certain shapes this can give the user more control over the way the shape flows.

test
Sweep between spans checked ✓
test
Sweep between spans un-checked

Fill center of inner closed vector rails

If you are sweeping two closed vectors to form a border or boundary shape, you can have Aspire automatically find the height that the cross-section forms on the inner boundary and then fill the shape to this height. To activate this check ✓ the Fill center of inner closed vector rails option in the form. This tool is perfect for sweep decorative bases, plaques or stands. Below left you can see a shape created with this option off and on the right an option with it activated.

test
Fill center un-checked
test
Fill center checked ✓

Smooth transition through the Cross Sections

As the swept shape passes through each cross section the default is for it to flow smoothly through the profile. This can be edited by right-clicking over the end node of the cross-section and unchecking the Smooth option.

test
Smooth checked ✓ on all cross sections
test
Smooth un-checked on all cross sections

Scale to Exact Height

Checking ✓ this option scales the shape calculated so its maximum height is the value entered in the Height area of the form.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

Job Setup - Double Sided

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

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

Job Type

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

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

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

Job Size

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

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

Z Zero Position

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

Zero off same side

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

XY Datum Position

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

Aspire has two smooth joining methods:

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

Create Job Sheet

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

Auto Open

If you wish to automatically open the Job Sheet after creation, simply hold down the CTRL key on the keyboard as you select the Create Job Sheet option from the menu.

Each job sheet document comprises the following information:

Job Layout

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

Material Setup

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

Toolpaths Summary

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

Toolpaths List

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

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

test
Selected Vectors
test
Circles Copied along curves

Distance between copies

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

Number of copies

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

Align Objects to curve

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

test
Selected Vectors
test
Stars Copied along the curve

Create Copies on new layer

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

Reverse Direction

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

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.

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. Aspire 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.

Save All Visible Toolpaths as a Template

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

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

Multiple Sheets

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

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

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

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

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.

Create Shape

The Create Shape tool allows the user to create Components based on one or more closed vectors. The vectors can be selected either before the icon is clicked or after the form is open. The user works through the form specifying the profile and strength of the shape and modifying options to govern its height. There is also an option to Tilt the shape on an angle. Once any of the parameters have been defined the shape can be previewed by hitting .

This shape can be easily changed by altering the parameters in the form and hitting the button to update the preview. Once you are happy with the shape created then you have two choices, to (which will save your current component and start a new one) or the form.

Changing values with the sliders on the form will immediately update the 3D view when you release the slider. If you make changes to the edit fields such as Angle or Base height, pressing the 'Space' bar on your keyboard after you have finished entering your value will apply the changes and update the 3D preview or you can hit the button again.

If you select another vector, then the current shape will be discarded, so remember to hit if you want to keep a copy of it.

Shape Profile

There are six different shape types:

Curved

Angle

The Angle setting will define the angle of the edge of the rounded or angled profile shape - the higher the angle, the steeper the shape. Angular shapes can have a maximum angle of 89°. The slider bar to the right can also be used to change this as well as typing a specific angle into the form.

Concave

S-Shaped

Flat

Custom

The custom shape profile uses a vector to define the profile rather than using one of the standard profiles.

To use the custom profile option a selection of closed vectors, plus an additional open vector representing the profile, must be selected.

When using a custom profile, the form the final shape will take comes from considering the shape above the line joining the end points. For this reason the profile vector should usually have a leg.

test
Profile with leg
test
Result of profile with leg
test
Profile without leg (left) and how this profile is interpreted by the software (right)
test
Result of profile without leg

Base Height

Specifies the height of a flat 'base plane' added below the profile you have chosen.

Final Height

No Limit

Checking ✓ this option lets the combination of the size and shape of the vector and the specified profile values govern the final height of the shape.

Limit to Height

Checking ✓ this option limits the height of the shape by flattening it off at the value entered in the Height area of the form which becomes active once this option is selected.

Scale to Exact Height

Checking ✓ this option limits the height of the shape by scaling the shape up or down while retaining its general specified profile. It is scaled to the height entered in the Height area of the form which becomes available once this option is selected. The slider can also be used to change the final height.

The Base Height value is not included or controlled by the Final Height setting and if specified will be added to this value to give the total height of the component being created.

Blend To Inner Vectors

This option applies the selected profile across the selected vectors. It blends to the profile from the outside of the vectors to the inner vectors

test
test

Sweep

The sweep option takes the profile chosen and sweeps this profile around the selected vector, blending the profile inwards, but not distorting the original profile. This is particularly useful when used in conjunction with the custom profile.

Tilt

When this option is checked ✓ the user can set a direction and angle to tilt the shape up at an angle in Z. The first part of this operation (once the option is checked ✓) is to press the button - then click two points in the 2D view.

The first click specifies the point which will remain at zero (the pivot point of the tilt).

The second click specifies the point that will be tilted upwards by the specified angle (the point that will be raised up).

The default angle (10°) can be edited by clicking the arrow next to the value and using the slider or by typing in a specific value and hitting the Space Bar on the keyboard to apply the angle.

Common Modeling Options

All of the main modeling tools in the software use a common set of commands to assign a name and combine mode to the component being created along with options to apply the settings in the form, reset the shape, start creating a new component and close to exit the function.

Combine with other components...

This section includes options to allow you to name your Component and control the way it will be combined with other objects in the Component Tree.

Reset

Clicking the button will remove the current shape, doing this before you Close the form will ensure that a component is not created from the current selection. Clicking this does retain the current set of selected vectors or Components.

Apply

Clicking the button will create a shape based on the settings you have chosen. You can continue making edits to the component by choosing different parameters within the form and hitting Apply to update it.

Start New Component

Clicking the button will save the state of the component that has been created, deselect all components/vectors and start the creation process again on a new component. The values and options within the form will be retained in this case until you Close it.

Close

Clicking the button will close the form returning to the Modeling Tab icons and the updated Component Tree, reflecting any changes that you have made. If you wanted to remove the shape you just created then you can hit the Undo icon or use the keyboard shortcut to undo, CTRL+Z.

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 ✓.

test
Offset Boundary only
test
Offset Boundary and Rubber Band together


Export Model as an STL File

The STL file format is an industry standard for representing 3D models as meshes made up of a skin of triangles. It is a very robust way of exporting a version of your 3D composite model to external applications or even Rapid Prototype (RP) machines. Models can also be exported as an OBJ file, which includes the component colors and is primarily used for ray-traced rendering of your model.

Limit Triangles By...

In general, triangle meshes are not able to hold as much detail as Aspire's 3D Components. As a result, you must choose which strategy Aspire will use to reduce the detail in your STL file.

Note

When exporting the rotary model, currently there is no control over the number of triangles and the mesh will be exported at the highest quality. That means that the generated file will have a considerable size.

Approximate tolerance

Using this option the quality of the mesh is defined by how closely you allow the software to approximate the model. The smaller the number the better the detail and smoothness of the model but the larger the memory size of the file will be.

Maximum number of triangles

Using this option the quality of the mesh is limited by how many triangles you specify here, the larger the number the better the detail and smoothness but the larger the memory size of the file will be.

Back face of triangulation

The Composite model does not have a defined back face, because it is generally unnecessary for conventional 3-axis CNC machining. When converting your composite model to a 3D mesh, however, it can be useful to form a closed mesh by creating a back face automatically.

Leave Open (No Back Face)

This creates a mesh with an open back. This creates a shell with the 3D shape on its face and an open back side.

Note

When exporting the rotary model this option will result in a mesh without caps at the ends.

Close with inverted front

This creates a mesh with a copy of the front of the model on the back. This is used when a solid 2 sided model is needed for output. An example of this might be a 2 sided fish.

Note

When exporting the rotary model this option is not available.

Close with a flat plane

This creates a mesh that has its back sealed off with a flat plane. This type of closed model may be required by Rapid Prototyping (3D Printing Software) to allow the part to be prepared for the production process.

Note

When exporting the rotary model this option is not available.

Close with other side (two-sided jobs only)

In the case of two-sided jobs, this option can be selected. It will triangulate both sides of a job and produce a single closed mesh.

Note

When exporting the rotary model this option is not available.

Close sides

This option is only available for rotary jobs. When it is selected the created mesh will have caps on the ends.

Triangulate

When the options for the mesh have been selected then clicking will actually calculate the mesh and display the result in the 3D View. If this does not look correct (such as not being detailed enough) then the options can be changed and this button clicked again to re-calculate the mesh.

Num Tri Created

Once a mesh has been created, this field reports how many triangles it comprises. The more triangles are used, the larger the file size and the more difficulty external applications may have in manipulating them.

Maximum Error

This field indicates the worst deviation of a mesh triangle from the original 3D model.

Draw shaded triangulation

The triangle mesh can be viewed in wireframe or shaded modes using this option.

Save Triangulation...

Once the mesh looks correct, then clicking this button enables it to be saved onto your computer as an STL format file by default. The file save dialog also allows the selection of Wavefront (*.obj) and POV-Ray Scene (*.POV) as an alternative triangle mesh format using the Save as type option.

Note

When saving an obj file, an additional material (*.mtl) file and texture image file (*.jpg) will also be created - all three files will be required when opening the obj file in a 3rd party modelling or rendering package.

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,

  1. POST_NAME
  2. UNITS
  3. LASER_SUPPORT
  4. Various variables
  5. The HEADER section

We have to ensure that those things are kept the same in the new Next_Wave_CNC_mm.pp.

Steps

This will serve as a rough set of steps on how to approach this.

  1. Create a new empty file (called Next_Wave_CNC_mm_2.pp, for example) and copy the contents of the Next_Wave_CNC.pp into it.
  2. Go through the old inheriting post-processor (Next_Wave_CNC_mm.pp) and copy / replace the variables and sections.
  3. For example, replace POST_NAME, UNITS and LASER_SUPPORT

The beginnings of the new post-processor should look something like this

POST_NAME = "Next Wave CNC (mm)(*.tap)"
FILE_EXTENSION = "tap"
UNITS = "MM"
DIRECT_OUTPUT = ""
SUBSTITUTE = "({)}"
LASER_SUPPORT = "YES"

Keep going and replace / add the variables (starting with VAR).

Replace the begin HEADER section.

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!

Emboss Component

Embossing a component can be used in some cases to reduce the height of a model while preserving important surface detail as an alternative to the standard method for scaling a components height using the Shape Height option on the Component Properties form. A component must be selected before the tool can be used.

The images below show the same model, both results are scaled to ten percent of their original heights. The image below left was created using the standard Shape Height scaling from the Component Properties form and the image below right using the Emboss function.

test
Original model
test
Embossed Model

Scale Height

Use the Scale Height slider to adjust the final height of the component.

Detail Smoothness

Since the results of the initial detail scaling can be noisy the Detail Smoothness slider can be interactively adjusted to improve the visual quality of the result. In general, the greater the Scale Height the more Detail Smoothing needs to be applied.

Remarks

The Emboss tool is a very powerful feature but will not provide ideal results on every type of 3D model. Although it's possible to use the Emboss tool on models created in Aspire and other low-relief imported designs (such as the clipart), it's important to understand its intended use is with data from imported, full 3D (high relief) models and typically the best results will be obtained with this type of data.

Toolpath Templates

Toolpath templates allow you to improve the efficiency of your production processes by saving the complete toolpath settings for common operations. These settings can then be re-used at any time on different design geometry. Frequently used strategies and tooling can thus be applied to similar jobs, quickly and easily.

The operations you can do with templates include Loading toolpaths from templates, Saving a toolpath to a template and Saving all visible toolpaths to a template.

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

Create Component ►

Create Component From... ►

Create Component from Bitmap

Import Component / 3D Model

Export as STL

Export as Grayscale Bitmap

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

Sculpt Visible Model

Smooth Selected Components

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

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

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

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

Emboss Component

Scale Model Z Height

Distort Selected Component

Replace Below

Selected Component Properties

Create Component

Create Shape From Vectors

Two Rail Sweep

Extrude and Weave

Turn and Spin

Create Textured Area Component

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

Export As Grayscale Bitmap

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

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

test
Composite Model
test
Saved Grayscale image

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

Create Component from Toolpath Preview

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

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

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

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

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

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

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

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

test
Standard Component
test
Shift Key held
test
Ctrl Key held

IMPORTANT NOTE

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

Array Copy Toolpath

Using the same approach as the Array Copy Tool for vectors in your drawing, this toolpath operation allows you to duplicate one or more toolpaths into a grid of copies. One of the key benefits of this approach is that it allows you to subsequently edit your original toolpaths and the software will automatically update the associated array of copies.

Toolpath Selection

To use the Array Copy Toolpath, open the form and turn on the visibility for each of the toolpaths you wish to be part of your array using the visibility checkbox next to each toolpath in the list below the form. The current selected toolpaths appear in the Toolpaths list at the top of the form.

The position of the resulting grid of toolpaths is always created to the right and above the source toolpaths. Therfore, you should always position your source toolpaths in the bottom left corner of the area you wish the array to fill.

Rows and Columns

Use the Rows (Y) and Columns (X) boxes to specify the size of your grid and thus the total number of copies of the original toolpath(s) that will result.

Spacing

The spacing between the copies of the toolpath within the grid are controlled using the Offset and Gap radio button options. The X and Y edit boxes determine the offset between the start point of each toolpath or the spacing between the bounding boxes of the copy, depending on the radio button option selected.

Minimize Tool Changes

The final option, Minimize tool changes, will only be available if the source toolpaths are using different tools. This will group toolpaths with the same tool geometry across the copies so that they can be output together. By grouping in this way, the parts of each copy using the same tool are cut together and the entire array can be cut with the minimum number of tool changes. If this option is not set, then the toolpaths for each copy will be cut individually, with tool changes required for each. See the The Array Copy Toolpath Cut Sequence

Working with Array Copy Toolpaths in the Toolpath List

Array Copy Toolpaths are displayed in the Toolpath List in different way to other toolpaths. The source toolpaths (the ones originally selected as the basis of the array) are now shown below the array copy toolpath item in a tree structure. For complicated jobs you can hide the source toolpaths in the list using the small and controls next to the Array Copy Toolpath in the Toolpath List. The usual visibility checkboxes are also available for both the array copy toolpath and its source toolpaths.

You can rearrange the order of the source toolpaths within the array copy group either by dragging them up or down using the mouse, or by click the up and down ordering arrows at the top of the Toolpath List. These features give you total control of each toolpath type within the array and are particularly important for saving the toolpaths

Saving an Array Copy Toolpath

As far as possible, array copy toolpaths are saved in exactly the same way as other toolpaths except that each source toolpath in the list represents all of its copies. If you switch off the visibility of a source toolpath before saving, noneof the copied instances of that toolpath will be included in the saved toolpath. Thus you can use the visibility controls to save a toolpath that will cut all of the copies, but limited to a particular subset of the source toolpath types.

In general, the sequence of cutting will be to cut all of the included toolpath strategies for each copy in the grid before moving on to the next copy.

Important

If the array copy toolpath contains more than one source toolpath using the same tool, then the sequencing within the array copy toolpath as a whole can be affected by the Minimize tool changes option setting when it was first created.

Baking Components

In general, the most useful feature of individual Components is that they can be manipulated entirely independently of each other to build up simpler design elements into a sophisticated 3D model. There are some editing functions that require the individual element to be consolidated into a single object. For example you may wish to smooth one shape into another using the sculpting tools or bend a group of Components around a curve using the distortion tool. In Aspire, consolidating a selection of Components into a single, new object is a process called 'Baking'. Once baked, the selected Components will become a single Component object and you will no longer be able to access the individual elements.

Aspire will prompt you when you have a group or Component selection that requires baking before a particular modeling tool or operation can proceed. Alternatively, you can use the Bake command to perform this operation yourself. By manually baking-in existing fade, tilt or distortion, for example, you are then free to apply further dynamic properties 'on top of' the previously applied ones. In addition, consolidating multiple Components towards the end of the design process allows your computer to recover system resources and may give it a welcome performance boost - particularly if you have been modeling using a large number of high resolution or complex Components.

Copy

If you hold the Ctrl key down when you hit the Baking icon it will retain a copy of the original Components and create a new baked Component instead of replacing the original selection.

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