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.

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

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

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

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

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

Exploded Flat Layout

Three Views - Front, Top, Side

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

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

Part Orientation

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

Auto Orientate

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

Orientate by material

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

Gap between parts

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

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

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

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

Options Checked ✓

Options Unchecked

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

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

A SketchUp model will often contain parts that you do not wish to machine (such as hinges, knobs etc.) or data which will be cut from different thicknesses of material and hence different parts need to be imported into different Aspire for ALPHACAM 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 for ALPHACAM. The screenshot below shows the result of only importing data on the 'Door' layer from the example.

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

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

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

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

Although when can treat this as a single 'part' when imported by starting its name with __ (two underscores), the imported part is still going to be difficult to machine. The screenshot below shows the part imported into Aspire for ALPHACAM 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 for ALPHACAM 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 for ALPHACAM 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.

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.

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

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

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

When this option is ticked,

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

Tapered column with distorted clipart

Tapered column with clipart stretched to overcome distortion

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

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

This section will present a 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 Use Selection button. The rails will be highlighted. Then select the profile vector and click apply. Inspect the 3D view to verify the results.

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

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

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

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

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

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

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

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

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

Heart-shaped vector and its unwrapped version

Extruded heart shape

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.

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

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

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

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

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

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

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

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

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

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

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

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

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

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

Bend Text Upwards

Bend Text Downwards

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

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

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

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

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

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

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

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

Rotate Copies selected

Rotate Copies not selected

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

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 Apply to create your 3D turned shape.

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

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 Apply to create your 3D spun shape.

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.

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

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

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

Clearance less than Tool Diameter

Clearance greater than Tool Diameter

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

No Border Gap

Border Gap

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

Rotate Parts Enabled

Rotate Parts Disabled

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

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

Original

Parts Nested inside other parts

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

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

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

Double-sided part before selection

Double-sided part when selected

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

Along X

Along Y

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

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.

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).

Checking ✓ this option will let you define a particular value for each slice. Right below this the Number of Slices will be displayed which is determined by the Composite Model thickness divided by the Slice Thickness. The model will be sliced from the bottom up and if the Composite Model thickness does not divide exactly by the Slice Thickness then the top slice may not be a whole number. To help indicate how the part is going to be divided the Top Slice Thickness is displayed in the form.

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

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

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.

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

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

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

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

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

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

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

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

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

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

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

Loose

Tight

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

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

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

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.

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

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

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

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

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

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

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

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

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

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

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

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

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

Aspire uses following workflow that covers both of those cases:

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

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

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

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

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

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

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

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

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

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

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

The 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.

3-axis rotary machining, tool correctly positioned

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

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

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

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

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

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

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

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

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

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

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

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

Make sure that Imported model type is set to Flat model

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

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

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

Each rotation can be undone by pressing Ctrl+ Z.

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

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

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

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

In the unfortunate event of the software crashing,

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

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

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

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.

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

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:

The distance between the text and the bounding box where:

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

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

No Vertical Stretch

Stretch Line Space to fit

Stretch Characters to fit

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

No Horizontal Stretch

Stretch Spaces between words

Stretch Kerning (space between letters)

Stretch Character size

Rectangular Border

Oval Border

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

Rectangular Border

Oval Border

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

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

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

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

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

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

Example

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

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

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

Examples

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

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

• Click Create to update the star.

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

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

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

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

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

After logging in here with your V&Co account details another page may appear asking for permission for Aspire for ALPHACAM 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 for ALPHACAM to retrieve your license details automatically.

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

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

This page displays the selected license and module details. If you are changing current license details or adding a module a restart will be required for these to fully take effect. In this case a check box will appear allowing you to restart automatically. If this is checked then when you press Finish Aspire for ALPHACAM 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 for ALPHACAM is restarted.

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

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

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

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

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

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.

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

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

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

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

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

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

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

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

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

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

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

To enter text:

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

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

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

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.

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

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

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

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

Vectors are lines, arcs and curves which can be as simple as a straight line or can make up complex 2D designs. They have many uses in Aspire for ALPHACAM, such as describing a shape for a toolpath to follow or creating designs. Aspire for ALPHACAM 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 for ALPHACAM supports the following vector formats for import: *.dxf, *.eps, *.ai, *.pdf, *skp and *svg. Once imported, the data can be edited and combined using the Vector Editing tools within the software.

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

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

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

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

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.

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

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

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

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

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

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

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

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

Toolpath for coves of the column

Toolpath for flutes of the column

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

Although the design can be considered to be finished, in practice it is useful to be able to cut-out the remaining stock. This can be realized by making the design slightly longer and adding profile cuts. In this example the blank length was extended by 2 inches using the Job Setup . Existing vectors can be recentered using F9. After 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. Cutout toolpaths and the resulting simulation has been shown below.

Cut-out toolpaths in 2D view

Finished part after adding cut-out toolpaths

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

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

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

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

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

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

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

Vectors used to create spiral flutes

Spiral toolpaths in flat view

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

Snap to Nodes, mid-points, centers

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

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

Snapping lines can be drawn from:

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

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

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

Bounding Box

Object Center

Nodes

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

Vectors

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

Vertical

Horizontal

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

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

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

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

If you have the job snapping

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.

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.

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.

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.

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

Add

Subtract

Merge

Low

Group

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.

Components can be selected in 3 ways:

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

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

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

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

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

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

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

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

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

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

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

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

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

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.

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.

The quickest and simplest way to draw an ellipse is:

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

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

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

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

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

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

Examples

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

To edit an existing ellipse:

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

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

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

Editing Modes

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

The three editing modes are:

• Vector Selection
• Node Editing
• Interactive Selection

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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.

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.

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.

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

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

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.

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

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

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

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.

All the objects assigned to a layer can then be simultaneously selected, labeled, colored, temporarily hidden or even locked (to prevent accidental editing) using the Layer Management tools. Even for relatively simple designs, organizing the elements of your artwork onto layers can make managing your project much easier.

Each layer in the list has five elements:

Status Icon

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

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

Layer Colour

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

Layer Content

The layer content icon will be grayed-out as an additional indicator that the layer is not currently visible. Layer Empty Content Icon a blank white sheet indicates that the layer does not currently contain any objects or vector geometry. If you import files from 3rd party CAD drawing packages via DXF or DWG format it is common for the file to include empty layers. This icon allows you to identify these empty layers and delete them.

Layer Name

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

Pop-up Menu

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

Select All on a Layer

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

Layer Ordering Arrows

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

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

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

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

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

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

Alternatively Gagdets can be assigned shortcuts.

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

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

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

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

Wrapping Sub-menu:

• Wrapped Fluting Layout
• Wrapped Spiral Layout
• Rounding Toolpath

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

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

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

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 Preview button to see the results of the offsetting.

Click OK to proceed or click Cancel to exit the form.

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

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

Original model

Negative Offset

Positive Offset

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

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

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

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

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

Example

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

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

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

Examples

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

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

Click Apply to update the circle

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

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

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

The data to be entered falls into three separate categories.

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

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

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

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

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

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

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

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

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

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

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

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

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.

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

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

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

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

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

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

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

Will retain any sharp corners in a design.

Offset with Sharp Corners on

Offset with Sharp Corners off

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

Using Vector Unwrapper with the star-shaped vector

Rails and uwrapped star

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

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

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

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

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

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

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

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

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

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

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.

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 Use Selection 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 Reverse Rail 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 Swap Rail Order 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 Make Start Point or you can right-click anywhere on the vector and select Insert Start Point to create a new node which will become the start point.

The Clear Rails 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.

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 Apply button to create your 3D swept shape.

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

Adding Cross Sections

Result From Two Rail Sweep

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.

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.

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

Scale cross section with width un-checked

Scale cross section with width checked ✓

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

Sweep between spans checked ✓

Sweep between spans un-checked

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

Fill center un-checked

Fill center checked ✓

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

Smooth checked ✓ on all cross sections

Smooth un-checked on all cross sections

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.

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

Aspire for ALPHACAM has two smooth joining methods:

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

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.

Enter the diameter of the required circles

Selected Vectors

Circles Copied along curves

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

Selected Vectors

Stars Copied along the curve

This tool allows you to easily select vectors which meet a set of criteria, such as open, closed, circular and also matching constraints based on layers. The dialog can be accessed from the Edit ► Vector Selector menu item, or from the Selector... button on each toolpath form. When the command is executed the dialog shown is displayed.

The dialog is used to configure a set of 'filters' that determine which vectors will be selected. A filter is enabled by clicking on its check box, or selecting a 'radio button' option, the current selection will be updated with all the objects in the file which match the current filter options.

Generally you will start at the top of the dialog and work downwards, specifying more and more explicit filters to determine the required selection exactly.

The simplest option is just to use the form to Select Closed Vectors in the job or Select Open vectors (you can specify both, in which case all vectors will be selected as long as they are on a visible layer).

The most common way to use the Vector Selector is to select all the vectors on a given layer as shown in the screenshot of the dialog below.

By associating a template with the result of a Vector Selector filter, we can make a template to automatically select the vectors it is intended to machine. A simple case would be to create a template which consisted of a Pocketing toolpath set up to machine all closed vectors on a layer called Pocket. After loading this template into a new job and choosing Toolpaths ► Recalculate All Toolpaths , the toolpath would be recalculated automatically selecting all closed vectors on the layer called Pocket.

The advanced templates are created by selecting the vectors for a toolpath using the Selector... button on the toolpath form. When a toolpath form is first opened, the Vector Selection: section on the form will show that vectors are being selected manually as shown below...

Pressing the Selector... button will display the Vector Selector form as shown previously. After making your geometry selection and before you close the form, select the Associate with toolpath option on the form as shown below.

After the Vector Selector form closes, the Toolpath form will indicate that Vector Selection is now 'Automatic' as shown below...

When you re-calculate or edit a toolpath that has the Vector Selection mode set to automatic, the vectors which match the filter when the toolpath is re-calculated or edited will be selected. To cancel the Automatic vector selection mode, you can just select the vectors to machine normally with the mouse, or use the Selector... button to bring up the Vector Selectordialog again (the settings are remembered) and uncheck the Associate with toolpath option.

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

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

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

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

The 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 Apply.

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

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

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.

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.

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

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 Set Anchor 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.

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.

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

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

	Turn horizontally from left to right
	Turn vertically, end over end

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

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

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

Toggle Two-Sided View

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.

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

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

Offset Boundary only

Offset Boundary and Rubber Band together

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.

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.

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

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.

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.

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.

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.

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

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

Original model

Embossed Model

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

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

Composite Model

Saved Grayscale image

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

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

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

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

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

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

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

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

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

Standard Component

Shift Key held

Ctrl Key held

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 for ALPHACAM 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.

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.

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

Selecting the Linear type will create a ramp which is a diagonal line (following the vector) from the Start Depth to the Flute Depth. Below you can see a Linear Ramp Type shown from the side. This ramp is set to only ramp from the start and to go 50% of the flute length.

Selecting the Smooth type will create a curved ramp (following the vector) from the Start Depth to the Flute Depth; this will smoothly transition from the ramp into the full depth of cut. You can see an example of this shown in the image below.

This gadget is used to simplify the task of creating toolpaths to machine flutes and coves on a rotary work piece. The gadget is designed to be used in a rotary job

This gadget does NOT create toolpaths directly. It lays out vectors in the 2D view which can then have toolpaths created using either the Profile or Fluting toolpaths within the main program. The top part of the form allows the user to specify how many flutes to create and how far from the start and end of the work piece the flute should start and end. Flutes are laid out evenly spaced based on the circumference of the cylinder. If the user chooses to create coves at either or both ends, extra vectors will be created which can be machined with the Profile toolpath and the Machine Vectors On option to create the coves.

The bottom section of the form contains details about the cylinder dimensions and is presented for reference only.

After the gadget has run the vectors required for machining will be visible in the 2D view. If you have a 3D form for your rotary piece, you can use the Project toolpath onto 3D model option on the toolpath forms to have your fluting toolpaths follow the work piece surface.

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

Before Fitting

After fitting

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

Fitted with Bezier spans

The same bezier spans in Node-edit mode

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

The vector before fitting

The same vector fitted with straight lines

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

Initial Vectors

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

Once the 2D design is ready, 3D components can be created from 2D Vector drawings. This will probably involve adding and changing 2D artwork a bit as the 3D design evolves, so Aspire for ALPHACAM's interface makes the drawing and modeling tools easily accessible.

In addition, existing 3D models can be imported to be incorporated into a design, these could be files previously created in Aspire for ALPHACAM, 3D Clipart that has been purchased and downloaded or models from other CAD design systems in a supported format.

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

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

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

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

Minimum variation

Maximum Variation

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

Short wavelength

Long wavelength

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

Small amplitude

Large Amplitude

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

No noise

Medium noise

High noise

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

• Single Sided
• Double Sided
• 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.

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

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

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

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

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

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

Choose one of the 6 options to determine the most suitable direction on the model that defines the top surface (upper Z) that you want to use when it's converted into a Component.

You can also use the five options for Rotation about Z Axis to modify the position of the part being imported at this stage.

Applies the values you have entered for the X, Y or Z dimensions.

Many mesh files do not inherently have the units that they were made in embedde in the files, so the software is not able to tell if the files are supposed to be inches or metric, they will just have a particular value. Therefore it is quite common to need to scale the part from inch to metric or vice versa. If you import your model and you wish to work in inches and the file seems very large or if you work in Metric and the file seems very small then you will probably need to use the Scale mm/inches option. The next two items on the form cover this need.

Choose the unit of measurement (mm or inches) that you are working in, within the part the file is being imported into.

Changing the units will result in resizing the model. For example, if you had 5x5 mm dimensions, they would become 5x5 inches so the model becomes a lot larger.

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

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

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

This gadget is used to simplify the task of creating toolpaths to machine spirals (rope or barley twist) on a rotary work piece. The gadget is designed to be used in a rotary job

This gadget does NOT create toolpaths directly. It lays out vectors in the 2D view which can then have toolpaths created using Profile toolpath within the main program. The top part of the form allows the user to specify how many strands to create and how far from the start and end of the work piece the strands should start and end. Strand ends are laid out evenly spaced based on the circumference of the cylinder. The spacing between strands during spiralling can be controlled using either Spiral Pitch or Spacing between strands option. It is also possible to choose between right and left hand twists.

If the user chooses to create coves at either or both ends, extra vectors will be created which can be machined with the Profile toolpath to create the coves.

For machining both spirals and coves, Machine Vectors On option should be used.

The bottom section of the form contains details about the cylinder dimensions and is presented for reference only.

After the gadget has run it will display message saying how many revolutions will each strand made and the vectors required for machining will be visible in the 2D view. Please note that the vectors will be extending beyond the 2D boundaries of the job. That is expected and thanks to wrapping feature will end up producing spirals. Please refer to Spiral toolpaths

The Create Component from Visible Model feature allows you to quickly create a single component which is a copy of the model shown in the 3D View (the Composite Model). The new model created is placed on the active level.

It is common when working with lots of components to find that a number of levels have been used. If, as a final step, you want to edit the models using a tool like the sculpting (which requires the components to be baked together) then they all must be on the same level, however placing the models on the same level may change the appearance of the composite model. In this case we can use the Create Component from Visible Model tool. This resulting component may then be sculpted without any of the previous modelling information being lost.

Consider the following example of a lioness we are modelling, and all of its current levels.

Model Tree

Model

If we want to sculpt this model we must first bake it, but we currently can't bake it because the components lie on different levels. Also, baking them together will mean we lose all our structure that we have carefully built up losing the potential to edit the individual parts. So instead we use the Create Component from Visible Model tool. This creates a copy of what is visible. We can then bake this new component, and we can now sculpt without losing our structure

Model Tree after creating copy

Sculpted Model

The Create Texture Area tool assists in the creation of components with a repeating pattern or texture. It requires a single component and optionally one or more closed boundary vectors which define the region in which the tiling should take place.

The Create Texture Area form is accessed from the modelling tab.

The first step is to select the component you wish to be tiled. If you want to restrict the tiling to a region then you should also select one or more closed vectors which will represent the boundary when the texture is created. If no boundary vector is selected then the tiling will fill the entire job space.

The Create Texture Area form contains options to adjust the spacing, overlap, positioning and symmetry of the texture which are discussed below. When you click the Apply button then the software will create a Component based on the settings in the form and any vector you may have selected for the boundary.

At this moment the original selected Component will be made invisible to avoid confusion with what you can see in the 3D View.

Once you click Apply then this will effective fix the basic outline or silhouette of your Texture Area either based on the selected vector or the job area. It is possible to edit the size, position and rotation of this but if you wanted to change to a different border shape then you would need to start again with a new selection.

Seed Component

Tiled Result

By default the form has Transform Object selected at the top. In this mode you can click on the Texture Area Component and use the drag-handles to move, scale or rotate it. Note that this will not change the size of your Tile (original seed Component). To change the size of the Tile you would use the Edit Textured Area Component option which is covered further down in this document.

The spacing edit box or sliders can be used to control the degree of spacing between the tiles in a pattern component. You can adjust the spacing between the components horizontally and/or vertically. The amount of horizontal spacing is given in terms of a percentage of the width of the tile component. The amount of vertical spacing is given in terms of a percentage of the height of it. To control the amount of spacing, use the two sliders in the box marked Spacing. Drag and release the slider to set the percentage, or alternatively type an exact amount into the edit box above and either hit Apply or press the Space bar on the keyboard to update the result. You can enter both positive and negative values. Positive spacing values open gaps between the objects in the texture and negative spacing has the opposite effect making the tiles overlap one another as shown below.

Shape with -25% X and -25% Y spacing

The X/Y shift option can be used to move all the tiles in alternate rows horizontally or alternate columns vertically by the specified amount. As with the spacing, the X/Y shift is given as a percentage of the size of the component in the appropriate dimension and can be adjusted using either the sliders or the edit boxes. For example entering a shift value of 50% horizontally (X) would move the second row over by half the width of the object, the third row would be as the first, then the fourth shifted, this shift would also be applied to every other row after that within the Textured Area. Similarly entering a value of 50% for the vertical shift (Y) will move every other column up by half the height of the object.

Shape with 50% X shift

Shape with 50% Y shift

The reflection tool consists of four buttons. Each button represents one tile in a mini-group of four, starting from the lower left copy which is represented by the original Tile. Each button has 4 states of reflection, each time the button is clicked, the icon representing the button will change to show the current state. Click Apply to update the Texture Area Component with your new choice.

No reflection

Horizontal reflection

Vertical reflection

Both horizontal and vertical reflection

When you have created a pattern you can edit the size of the individual Tile component you are creating a pattern from by selecting the Edit Textured Area Component option at the top of the form. Within the 2D View this will then put an orange transform box around the lower left component in the pattern. You can alter the size of this by left clicking on one of the handles and dragging it to size, when you let go this will update the pattern to fit the new size within the Texture Area boundary. You can also move the location of this Tile by clicking the center node and dragging it with the mouse to a new location. This again will change the layout of the pattern.

Pattern in Edit Texture Area Component Transform Box Appears

Pull handle on Transform Box to Alter Size and the Pattern Updates to the New Size

A Texture Area component will remember that it is in a special state and not a standard component. This means that they can be further edited using the Texture Area form even after Closing and re-entering the function. To edit an existing Texture Area component, select it and then open the Create Texture Area tool. Alternatively, open the Create Texture Area tool and then select the existing component. This will then let you continue to make changes to it using the form.

Texture Area components do not behave like standard components when they are scaled in X or Y. When a Texture Area component is resized, then this resizes the boundary in which the tiling takes place so the size of the individual Tiles will not change, just the area that they are covering will be updated.

Typical baked component resize - shapes scale

Texture component resize - shapes do not scale

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.

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

To use:

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

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

Geometry before trimming. Select the lines first and then the circle

Trimmed vectors using Clear inside boundary

Trimmed vectors using clear outside boundary

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

Trimming with Group

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

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

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

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

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

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

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

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

This controls what the angle value does.

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

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

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

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

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

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

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

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

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

Example:

1 2 R Gives a radius of 12

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

Click Create to update the circle.

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

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

Click Apply to update the circle

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

To finish drawing with the tool, you can :

Click Close on the form

• Press the key Esc
• Click the Right mouse button in the 2D View

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

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

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

Straight Line Span Vectors before Filleting

Straight Line Span Vectors After Filleting

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

Vectors before Dog-Bone Filleting

Vectors after Dog-Bone Filleting

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

Vectors before T-Bone Filleting

Vectors after T-Bone Filleting

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

vertical edge clicked near the corner

Horizontal edges clicked near the corner

Fillets can be removed in the same way that we add fillets: move the cursor over the fillet that you wish to remove.

If this fillet can be removed then the cursor shows a cross to indicate that it is possible to remove a fillet:

Clicking removes the fillet:

Before removing fillet

After removing fillet

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

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

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

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

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

First click creates a preview extension line from the selected vector span.

Moving the mouse over another span will display a second preview extension line to the point of intersection. Click the line to apply this change.

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

This Gadget supports drag knife tooling in your CNC machine. It uses the selected vectors in the 2D View as the basis of a centerline profile-type toolpath that incorporates swivel moves at corners to ensure the drag knife blade remains properly aligned throughout the cut.

Each of the 5 sections of the Job Sheet can either be included or removed to display as much information as required. The image to the left, represents a default Job Sheet which includes the following 5 sections:

• Job Layout
• Job Notes
• Material Setup
• Toolpaths Summary
• Individual Toolpath Summaries

Files from Vectric's Cut3D, PhotoVCarve and Design and Make Machinist that include 3D toolpaths can be imported into Aspire for ALPHACAM using the main menu command: File ► Import ► PhotoVCarve, Machinist or Cut3D Toolpaths.

The 3D file must first be scaled to the required size before toolpaths are calculated, and then the complete file saved ready for importing into Aspire for ALPHACAM. These files can only be moved and positioned inside Aspire for ALPHACAM but cannot be scaled.

A Grayscale thumbnail of the 3D job is drawn in the 2D View with the X0 Y0 origin at the position it was set in Cut3D, PhotoVCarve or Design and Make Machinist. The associated toolpath(s) are also drawn in the 3D window and the names appear in the Toolpath list.

To move the 3D design toolpaths open the 2D Window, click the Left mouse Twice on grayscale image (turns light Blue to indicate it's selected), then drag to the required position, or use the Move or Alignment tools for accurate positioning.

The toolpath(s) are automatically moved in the 3D window to the same XY position as the image.

Origin for the 3D data at X0 Y0

Grayscale image moved to middle of job

Toolpaths for the example above have been calculated with the X0 Y0 in the middle of the 3D design. When imported into Cut2D the data is automatically positioned using the same coordinates, which places three quarters of the design off the job. In the second image the grayscale image has been moved to the middle of the job.

The 2D mirror and rotate drawing tools can also be used to edit the 3D data set.

3D toolpaths can also be copied using the Duplicate Toolpath command on the Toolpaths Tab making it very easy to use multiple elements from a single design on a job. The thumbnail preview is also copied for each toolpath, making it very easy to position additional copies of a 3D toolpath.

For example, a single design can be copied and mirrored to create Left and Right versions of a 3D design or to place multiple copies of a decorative design in the corners of a cabinet door panel as shown below.

Toolpaths for the 3D elements can be previewed along with the conventional Profile, Pocketing and Drilling toolpaths, and everything will be saved ready for machining.

A good example of where this functionality might be used in conjunction with PhotoVCarve is for making personalized picture frames that include the PhotoVCarve grooves plus descriptive engraved text and a decorative Profiled or Beveled border. As shown below:

2D window showing thumbnail previews, text and decorative border

3D window previewing the completed job

Imported toolpaths can also be edited to position them inside the material or to change the cutting parameters - speeds and feed rates can be changed.

Click the Edit toolpath icon or Double click on the toolpath name to open the edit form.

For example, after machining a half-inch deep pocket a PhotoVCarve design can then be edited to have a Start Depth = 0.5 inches and this will carve the photograph onto the base of the pocket surface.

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

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

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

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

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

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

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

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

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

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

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

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

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

Repeat for each of the Variable Names listed on the form

Click Calculate to create all Badges and associated Toolpaths

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

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

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

Unless otherwise noted below, dimensions are created by following these steps:

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

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

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

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

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

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

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

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

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

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

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

Vector selection methods

Multiple vectors can be selected in the following ways:

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

Deselecting Vectors

Selections can be cancelled by:

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

Numerical edit boxes generally support simple calculations.

A sum can be entered directly into the edit box:

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

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

For some applications it can be useful to eliminate vertical walls on 3D models, especially if the machined part is intended to be used as the basis for a mold or vacuum forming tool.

The Add Draft tool will automatically add a minimum angle to any steep walls that exist in your model. The draft angle is specified by using the slider or entering a typed value in the form.

When the Apply button is pressed, the tool creates a new 3D Component by baking the visible Components and applying the draft angle across all the walls of the composite model. Note that you do not select the Component/s to apply the draft angle to, just ensure that they are visible in the 3D view. The resulting Component will not have any wall angles that are steeper than the specified draft angle. Once complete, both the original Component/s and the new Component will be visible, although the original may be obscured by the new Component. The Component with the draft angle will be named appropriately indicating the amount of draft that was added. The images below show how a Component looks before and after adding 20° of draft.

Original Model

With Draft Added

This command opens the File Open dialog window, allowing existing Aspire for ALPHACAM files (CRV3D extension) and importable 3rd party 3D files to be selected and opened. If you select a 3rd party 3D model format, the Orientate Model form will open (see below) to allow you to manipulate the 3D model before it is converted into a Component.

When one of these formats are chosen for 3D file Import, the imported model needs to be oriented and scaled before it can become a Component. A special import window is opened and a set of orientation/scaling tools enabled. Depending on the job type, import window will be different:

• Importing a 3D Model into Single or Double Sided job
• Importing a 3D Model into Rotary job

Often it is advantageous to apply a general smoothing effect over the whole of a component (rather than smooth a particular area with the Sculpting Tools). To use this tool, select the components you wish to smooth and then click the Apply smoothing filter to selected components icon on the Modeling tab. The form will appear and Aspire for ALPHACAM will take a few seconds to prepare the model for the smoothing operation. You will see a progress bar at the bottom of the screen while it is doing this.

One or more Components can be selected for Smoothing. If you select multiple shapes or a Component Group then the software will need to Bake your selection into a single Component, if applicable you should ensure you have a safe copy of your current Components before proceeding.

If you wish to smooth individual components one after another, potentially with different amounts of smoothing, you can do this by selecting one component, apply a suitable smooth filter value with the slider and then hit the Bake Current Smoothing button in the form and then proceed to selecting the next component you wish to smooth. When pick a new Component the software may take a few seconds to pick it and apply the smoothing filter to it at the default of 50% strength. If you do not click on the Bake Current Smoothing button before you select a new component then the effects of the smoothing will be lost on the previously selected component.

The 3D View can show you the current Composite Model (which is built from all of the currently visible 3D Components and Levels), the Toolpath Preview (a highly accurate 3D simulation of the resulting physical object that will result from your toolpaths called the Preview Material Block). Which of these is currently displayed will depend on whether or not you have a part which has 3D Components and Toolpaths or are just working on something that only includes 2D Data.

Whenever you have the Preview Toolpaths form open on the Toolpaths tab, the 3D View displays the Preview Material Block instead of the Composite Model. When this is closed if you are working on a part that only includes 2D data and 2D or 2.5D toolpaths it will continue to display the Preview Material Block. If your part contains any visible 3D Components then as soon as the Preview Toolpaths form is closed it will revert to showing the Composite Model in the 3D View and hide the simulation. In addition to these items, you can see line drawings of any calculated toolpaths in the 3D View. The visibility of these calculated toolpaths can be controlled from the Toolpath List on the Toolpaths tab using the check-boxes next to the toolpaths name. If working in a 2 Sided environment you can view both sides of a project in the 3D View using the Multi Sided View option.

Aspire for ALPHACAMhas been designed to work in a way which enables the user to easily create even very complex projects. In any situation, the best approach to producing something complicated is to break it down into smaller pieces until a level of simplicity is reached that can be understood and managed. In Aspire for ALPHACAMthis is achieved by letting the user work with pieces of the design which are combined to make the finished part. In the terminology of the software these pieces are called Components. To help organize the Components they are assigned to Levels. Step by step, Components and Levels can be created and modified until you have all the elements you need. In the images below you can see an example of how this might work. On the left you can see the separate component for a model of a bunch of grapes and on the right you can see these positioned to make the complete part - we call this resulting combination the Composite Model.

There is no limit to how simple or complex a Component or the Components on a Level can be (this is the user's choice). In the example shown, you can see that a model of a whole bunch of grapes may be made up of smaller individual components but they could also be combined to exist as one single Component (the assembled bunch of grapes) that could then be used to lay-out a more complex part with multiple bunches of grapes. They could also be organized so all the grapes were on one Level and leaf and stem on another to provide a different way of managing and manipulating the shapes. Each user will find a level of using Components and Levels they are comfortable with which may be dependent on the particular job or level of proficiency with the modeling tools.

An existing Component can be copied, scaled and have other edits carried out on it as an object. The user can also change the way it relates to the other Components, for instance whether it sits on top or blends into an overlapping area of another Component. The shape, location and relation of these pieces determine the look of the final part. As the job progresses, the user will need to create brand new Components or edit existing ones by adding new shapes, combining them with others or sculpting them.

Components can be created and edited by:

1. Use a modeling tool to create shapes from 2D vectors.
2. Import a pre-created 3d model - either a model previously created in Aspire or from another source such as a clipart library or a different modeling package.
3. Create a 'texture' Component from a bitmap image.
4. Use the Split Components Tool to break an existing Component into multiple pieces.

All of these methods are covered in detail throughout the training material.

As well as having its underlying 3D shape, each component also has a number of dynamic properties that can be freely modified without permanently changing its true shape. These include scaling of the Component's height, the ability to tilt it, or to apply a graduated fade across it.

These dynamic properties can always be reset or altered at any time during your modeling process, which makes them a particularly useful way of 'tweaking 'your components as you combine them together to form your final composite model.

The Combine Mode is a very important concept when working with 3D shapes within Aspire. The options for combine mode are presented when creating new shapes and also when deciding how Components and Levels will interact in the Component List. Rather than cover this in every section where it is applicable, it is worth summarizing the options here so the general concept can be understood.

When you have more than one 3D shape, such as the Component pieces of the design or where you have an existing shape and are creating a new one, then you need to have a way to tell the software how the additional entities will interact with the first. This can be an abstract concept for users who are new to 3D but it is an important one to grasp as early as possible. In Aspire this is controlled by a choice called the Combine Mode.

There are four options for this: Add, Subtract, Merge High, Merge Low.

As modeling is an artistic and creative process, there is no general rule to describe when to use each one. As a guide though you can assume that if the second shape's area is completely within the originals one then you will probably be adding or subtracting and if the shapes only partly overlap that you will probably use Merge or, very occasionally, Low.

The four options and their specific effects are described on the following pages. To illustrate the different effects a combination of an overlapping beveled square and a dome will be used. You can see in the image top right how these are arranged in the 2D View and how they overlap. Then you can see each individual shape in the images below middle and right. These shapes will be used to demonstrate the different Combine Modes. In every case the Dome will be considered the primary shape and the square is the secondary shape which is being combined with the first. In addition to the dome/square example some images of 'real world' parts will also be included to help to understand how these can be used on actual projects.

As well as working on individual shapes, the Combine Modes are also assigned to Levels. These will govern how the combination of all the individual components on one Level interacts with the result of all the Components on the Level below it in the Component Tree

When Add is selected, it takes the first shape and then just adds the height of the second shape directly on top of the first. Any areas which overlap will create a shape which is exactly the height of each shape at that point added together (see below)

Typically the add option is mainly used when the shape being added sits completely within the original shape, this ensures that the uneven transition where the parts only partly overlap (as shown in the example) do not occur.

The example above shows the Maple Leaf and border extrusion Components being Added to the dome Component in the sign example from the Introduction to Modeling document.

When Subtract is selected it takes the first shape and then removes the height of the second shape from the first. Any areas which overlap will be a combination of the original height/shape less the second shape. Areas where the shape goes into the background will become negative regions. You can see how this looks using the dome and square in the image below:

Typically subtract, like the add option, is mainly used when the shape being removed sits completely within the original shape, this ensures that the uneven transition where the parts only partly overlap (as shown in the example) do not occur.

The image shown above has some 'creases' to help define the muscles of the lioness. The shapes to create these recesses were created by using the Subtract option with the Create Shape tool on the vectors representing those recessed areas.

When the Merge option is selected any areas of the shapes which do not overlap remain the same. The areas that overlap will blend into each other so that the highest areas of each are left visible. This results in the look of one shape merging into the other and is in effect a Boolean union operation. You can see how this looks using the dome and square in the image below:

Typically the merge option is used when the shape being combined partly overlaps the original shape. This enables a reasonable transition to be made between them.

The image above shows 2 Herons, a rope border and banner Components. Each of these overlaps with the others and so they are set to Merge in this areas. Whatever is the higher of the two merged areas is what is prominent. In this case the rope is lower than everything and the Banner is higher than the Herons so the desired effect can be achieved.

The Low option is only available when combining Components (not in the modeling tools). When this mode is selected, any areas which do not overlap are left as they were in the original two shapes. Any areas which overlap will create a new shape which is the lowest points taken from each shape, this is in effect a Boolean intersection operation. You can see how this looks using the dome and square in the image below:

The Low option is used for recessing a shape into a raised shape. An example of this is shown in the image above.

The example shown on the right above uses the Low option to combine the flat topped 'button' component on the left with the curved top face component with the letter 'A' on the right. Combining both components with the merge low option gives the keyboard button with the curved top you see in the bottom row.

Right-clicking Levels in the component tree will open a pop-up menu offering commands and operations related to the clicked level and Mirror Modes can be set in this way. If a mirror mode is set on a Level, all the components it contains will be continually mirrored dynamically as they are moved, transformed or edited. The mirroring is non-destructive, that is it can be turned off or on at any time and does not alter the underlying components in any permanent way. Working inside a Mirror modes Level is a simple way of achieving a complicated symmetrical pattern by editing only one half (or quarter, see below) of the design.

The available Mirror Modes are broadly divided into two groups. The first group apply one plane of symmetry:

• Left to Right
• Right to Left
• Top to Bottom
• Bottom to Top

These modes allow you to work in one half of your job and the other half will be automatically and dynamically generated for you. For example, in Left to Right mode you would place your components in the left half of your job and a mirrored equivalent of each would be created in the other half of the job. This 'reflection' is updated dynamically as you work.

The other group offer two planes of symmetry (horizontal and vertical):

• Top Left Quadrant
• Top Right Quadrant
• Bottom Left Quadrant
• Bottom Right Quadrant

When using these modes your components should all be in the quadrant (quarter) of the job. Mirrored reflections horizontally and vertically will be created in the other quadrants of the job for you.

When working in a 2 Sided environment you can create components independently per side or using the Right click option you can copy or move a component to the opposite side. Selecting the option to work in 'Multi Sided View' allows you to view components you may have on the Top and Bottom side in the 3D View. In the Toolpath Preview form of a project that contains toolpaths for the Top and Bottom Sides the multi sided view presents the simulation of the toolpath preview on both sides also, if the multi sided view is not selected you can use the 'Preview all Sides' option in the Toolpath Preview form to display the Top and Bottom Toolpaths in the 3D view. 2 Sided Setup will be described in detail later in the relevant section of this manual.

The Sculpting function in Aspire for ALPHACAM is a very powerful way to edit (or create) 3D shapes. It allows the user to perform truly dynamic interactive editing of 3D Components. Once activated, the user chooses from a variety of tool options which determine how the model will be changed and then uses the mouse (or a pen tablet) to actually edit the 3D model. This is done in the 3D view and requires the user to click and move the mouse cursor in the area of the model they want to apply the tool. The best way to understand this tool is to actually try it and to watch the Tutorial Videos that are supplied with the software as it is very much a visual tool (which is what gives it its power).

One or more Components can be selected for Sculpting. If you select multiple shapes or a Component Group then the software will need to Bake your selection into a single Component, if applicable you should ensure you have a safe copy of your selection before proceeding.

In addition to components, you can also select bitmap. The bitmap will be overlaid on the sculpted model. This is useful when sculpting based on the photo.

As the user moves the mouse over any area of the 3D model that has already been sculpted then the area under the red cursor will be gradually returned to its original state. This can be used to undo some of the sculpting if you make a mistake.

Alternately you can use the Key combination Ctrl+Z to undo the last move that you made without using the Undo Brush.

Allow to quickly toggle between overlaid image being visible or not. This allows the user to work with overlaid image hidden and only displayed periodically to guide the sculpting process.

This option can also be accessed by pressing the O key.

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

• Click the left mouse button to indicate the start point of your line.
• Move the mouse pointer and click again to set the next point in your line.
• Repeat this process to add as many line segments as you require.
• Right-click or press Esc to finish your polyline and exit the form.
• Alternatively press the Space bar to complete this polyline but keep the form open and begin drawing another polyline.
• Press the Tab key to automatically close the vector.
• A smooth bezier span can be created by clicking and dragging to modify the curvature. The next span will then also be smoothed. If you want next line to be straight line then you can press S to disable the smoothing.

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

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

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

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

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

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

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

Examples

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

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

Examples

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

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

• The absolute X Y position of the next point
• The Angle and Length to the next point

The relative offset in X (dx) and Y (dy) to the next point.

Once you have entered the values you wish to use :

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

The Component Properties form allows you to adjust a number of dynamic properties for a selected Component or Level. Adjusting these properties does not make permanent changes to your Components and can be further edited or reset any time until the component is Baked, in which cases they will be made permanent in the Component shape and this form will be reset.

Adds the selected component/s to the result of all the previous components in the list.

Subtracts the selected component/s from the result of all the previous components in the list.

Where they overlap, this Merges the selected component/s into the result of all the previous Components in the list keeping the highest part of the overlapping area. This means the higher part of each shape will be what remains in this area.

Where they overlap, this Merges the selected component/s into the result of all the previous Components in the list keeping the lowest part of the overlapping area. This means the lower part of each shape will be what remains in this area.

Where there is an overlap, this Multiplies the result of all the previous components in the list by the heights in this component.

Use the slider or type in a specific percentage to scale the height of the selected Component(s) up or down based on its current height (100%).

Enter a value in the Shape Height edit box directly, or use the slider to adjust the height of your component selection interactively. In either case, the 3D view of the component will update automatically as you adjust the value. The range of available heights on the slider is determined by your current material thickness setting. If these values appear to be inappropriate you can still enter any value you like into the associated edit box, or you can close the tool and select Edit ► Job Size and Position from the main menu. In the Job Setup page you can then correct the current setting for the material thickness before continuing.

Enter a specific value into this box to raise the Component or Level up on a flat plane of the thickness you specify. This can be useful to help move an object up so it sits proud of another component it is Merging with. If you are not sure of the value you need, then enter an amount and hit the space bar to apply this. If this is not correct, type in another value and hit space again to apply the new value, look at the 3D View to judge the result - repeat until you get the value you need.

You can also apply a Base Height to a Level. Adding a base height to a level will add the same base height visually to the components in that Level, however the components themselves will have no base height added to them within their properties. This is useful to raise a set of objects on a Level above things that need to appear to be behind them (for example above a textured area).

Aspire for ALPHACAM gives you a lot of control over the appearance of the 3D shaded image for visualization purposes, such as customer approval proofs or marketing material. Each component can be given an individual color or material.

When this is selected the user can choose from the list of pre-defined material effects by clicking on the box immediately below the Appearance choice. These include many wood grains, metal effects, stone and plastic.

Additional materials can be added to the library. See Preview Toolpaths for more details.

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

Vectors Selected

Bezier node editing

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

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

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

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

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

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

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

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

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

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

When welding text, the internal regions of characters are preserved.

Overlapping text before welding

Overlaps removed by welding, but internal regions preserved

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

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

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

Will not change the size of the text block

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

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

Align to Curve

Keep Vertical

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

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

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

The Vector Validator is intended to help find issues with contours after file imports that are stopping tool-path creation such as overlapping contours or intersections. It also indicates zero-length spans.

The Vector Validator dialog can be opened with a selection to work on. If there is no selection, all visible vectors on the current Side of the current Sheet on visible layers will be validated. The selection can be changed while the form is open.

The text on the Search button changes to show whether all vectors or just the selection are going to be searched. While searching, the Search button becomes a Stop button.

To cancel a search, click the Stop or Close button.

Issues found so far will be marked.

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

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

When this option is checked, Vector Validator will perform its vector checks as it is executed and required for V-cutting.

For example,

• It will ignore intersections that may exist within the text, as this may be due to problems in the font. If you get intersections that involve text, you could try soldering it and run Vector Validator on the output.

Click on the interactive weave image to cycle through the different crossing options at each intersection point. The 3 options are:

• Cut Vertical
• Cut Horizontal
• Cut Neither

You can reset the Weave Preview Image at any time using the Reset Grid Content button.

When you are happy with the layout of the weave pattern, choose which cross-section you would like and clickCreate cross-section to add it to your 2D View.

Click the Apply button to convert the weave design you have created into vectors artwork in the 2D View. You can change the Weave Preview Image and click Apply to update this artwork as often as you like.

Click Close once you are happy with your design. The Celtic Weave Creator form will close, but if you re-select the unedited weave pattern in the 2D View and re-open the Celtic Weave Creator gadget it will reflect you currently selected weave in the Weave Preview Image for further editing.

To complete the weave process, open the Extrude and Weave tool on the modeling tab. Select the main weave pattern vectors (but not the cross-section vector) and click on the Use Selection button in the Drive Rails section at the top of the form. Now select the cross section vector and click anywhere on the weave rails vectors in the 2D View to apply the cross-section shape to it. Click Apply to create the weave.

There are many more options available to use the weave vectors created by this Gadget. For a full description, please see the section on the Extrude and Weave tool.

This tool converts one vector into another vector that can be used with the two-rail scanning tool to create rotational models from a desired cross-section.

To unroll the vector, follow these steps:

1. Select the contour you want to unroll
2. Use the options or the slide handle to select the center of unpacking
3. Press Apply

The generated contour can now be used with the two-rail scanning tool to create rotary models.

Sets the center of the job to be a specified point. The custom point can also be chosen by selecting the drag handle and dragging to the desired point.

The type of span you have clicked.
Possibilities include:

• Line
• Arc
• Bezier Curve

XY Drawing Origin - Here you can specify where the XY zero origin will be placed on your job. These options correspond to the same fields on the normal 'Job Setup' form within the program. Most people would use the default Bottom Left Corner, but for some jobs you may prefer to have the XY origin in the Center.

• In a job with horizontal orientation (Along X Axis), the X offset will correspond to the length of the cylinder, and the Y offset will be a point along its circumference.
• In a job with vertical orientation (Along Y Axis), it's the opposite. The Y offset will correspond to the length of the cylinder, and the X offset will be a point along its circumference.

Cylinder Orientation Along - This section is used to tell the program how you have your rotary axis aligned on your machine. If you've already made your design, but just want to change the job for a different machine, then you could flip your design with the material so that all the vectors and components stay the same relative to the job.

Z Origin On - This section determines whether the Z Origin is set to the surface of the material or the base (center of cylinder). These settings can be over-ridden when the toolpath is actually saved, but we would strongly recommend the 'Cylinder Axis' is selected for rotary machining. The reasons for this are detailed in the note below.

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.

As well as creating a job at a suitable size for wrapping toolpaths, when creating the job, it will create a number of vectors which can be very useful when creating your wrapped job.

The vectors are created on their own individual layers and by default these layers are switched off to avoid cluttering up your work area. To switch on the layers, display the 'Layer Control' dialog (Ctrl+ L is the shortcut to show / hide this). To show / hide the layer simply click on the check box next to the layer name.

2Rail Sweep Rails - This layer contains two straight line vectors which can be used to sweep a profile along if you are creating a shaped column.

Bounding Box - This layer contains a rectangular vector covering the entire job area. This vector is useful if you are going to machine the complete surface of the cylinder.

When setting-up rotary project, software assumes a perfect cylinder with an exact diameter. In practice the stock material may be uneven, or only blank with square profile may be available. In those cases blank needs to be machined into cylinder of desired size, before running toolpaths associated with the actual design.

Another consideration is length of the stock material. Typically, part of the blank will be placed within the chuck. It is also important that during machining, the cutting tool is always in safe distance from both chuck and tailstock. For those reasons, the blank has to be longer than the actual design. When setting-up the machine for cutting, one has to pay extra attention to ensure that origin is set accordingly to avoid the tool running into chuck or tailstock!

If the design was created without those considerations in mind, the blank size can always be adjusted in the Job Setupform.

The picture below presents an example of a rotary project layout. As explained above, the actual blank is longer than job defined in Aspire to allow for the chuck and sufficient gaps. The actual design is shorter than job defined in Aspire, to leave some space for tabs, that can be machined with the profile toolpath prior to removing the finished part from the chuck.

When machining 3D shapes with varying thicknesses like on the example shown below, it is a good idea to place the thicker end of the model on the side closest to the driving motor. This way torsional twisting will mostly affect the stronger end of the machined part and help to avoid bending or breaking of the part during machining.

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

Ungroup to the group's layer

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

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

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

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

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

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

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

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

• EPS
• DXF
• AI
• SVG
• PDF

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

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

The options to clear areas of a 3D Component, inside and outside of vectors or to slit a vector into multiple pieces are very useful modeling tools. There are many occasions where the standard modeling options may not allow you to create or control the exact shape that you need. Often you may need to create the general shape then crop (cookie cut) the resulting Component either to leave just the part of the shape you want or to make a hole in it. Many examples of this will be covered in the video tutorials supplied with the software.

Original Vectors

Selected Vectors with 2 Rail Sweep

Resultant Cropped component

In the image above and left you can see the vectors selected for a 2 Rail Sweep to make a simple flowing shape. The result of this sweep is shown in the middle image. Our actual leaf edge vector can be seen in the left hand image after cropping the swept shape back to the leaf outline vector.

To use the cropping function you need to select the Component or Components you want to edit first and then select the object last that you want to use as the cropping region. If multiple Components, or a Component group, are selected for this tool, Aspire will prompt for you to bake the Components before continuing. See Baking Component for more information.

This tool allows you to split the selected Component into two independent Components. To use this tool, you must select the Component you wish to split and a single vector to indicate the split boundary then click on the icon.

You can use either an open or closed vector to define the split boundary. A closed vector can be envisaged as a 'cookie cutter'. The resulting two Components will be as if the cookie cutter vector was pushed through the selected Component to split it.

If an open vector is used to define the split boundary, Aspire will extrapolate from the ends of the selected vector to the edge of the modeling area to create the two resulting split Components.

The names of the resulting Components are automatically appended with '- A' and '- B' in the Component tree.

If multiple Components, or a Component group, are selected for this tool, Aspire will prompt for you to bake the Components before continuing. See Baking Components for more information.

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

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

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

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

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

• View Toolbar
• 2D View
• 3D View

Select relative to the Material Surface or relative to the Machine Bed. This is a very important setting because the tooling used on the CNC machine must be setup in the same way, ensuring the toolpaths cut to the correct depth.

If you are working in a 2 Sided job, this will set the Z Zero for your current side only,

• The side you are setting up will be displayed in brackets e.g. (Top).
• You can set the Z-Zero for both sides through the Job Setup form.

The thickness of your model must be less than the thickness of the material you wish to cut it from. You can position your model within the material block wherever you wish by defining the gap distance either above or below your model. You can also double left click on either of the three lines next to the slider to position the model at the top, center or bottom of the material.

For all toolpaths, as well as specifying a rapid clearance gap for rapid positioning moves above the workpiece, the user can also specify a much smaller gap that the tool will rapid down to during plunge moves. By default the plunge gap is set to the same value as the Clearance gap which means that there will be no rapid plunges. If you set the plunge gap to a smaller value than the Clearance gap, the tool will plunge at rapid feed rate to the specified distance above the material surface before changing to the specified plunge rate. For jobs where a large value for Clearance gap has to be specified to avoid clamps etc, this feature can save a considerable amount of machining time if there are a lot of plunge moves in the job.

The Extrude and Weave feature is a very powerful and flexible modeling tool. It uses one or more vector drive-rails to define the path that the shape will follow, this allows you to extrude either vector cross-sections or 3D Components along these vectors to create the model.

The first stage is to select the drive rails and then choose whether you want to use either vectors or Components to extrude along your curves. There are many options both on the form and under the context sensitive right-click menus that can be used to control the shape that is created.

From the 2D View use the mouse to select one or more open or closed vectors you wish to use as the drive rails for you to extrude or weave along. Then click the Use Selection button.

In the 2D view your rail vectors will be highlighted orange and now show a green square (start node) indicating the start of the vector from which the extruded shape will begin, and arrow markers along its length to show the direction of the extrusion.

The default start point and direction shown may not be what you intended. To change the direction, right-click with the cursor on the vector line and select Reverse Rail from the context sensitive menu, you will now see the arrows on the drive rail change direction. On a closed vector you can change the start point by placing the cursor over an existing node in the drive-rail vector, right-clicking and selecting Make Start Point or you can right-click anywhere on the vector and select Insert Start Point to create a new node which will become the start point.

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

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

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

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

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

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

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

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

In some cases it may be advantageous to add a cross section at all node positions on a drive curve, for example on a closed rectangular border. This can either be done manually, or automatically after you have added the first Cross-Section by right-clicking on the cross section you wish to duplicate and selecting Add To All Rail Nodes. This will add that same cross section to every node on that specific drive rail vector.

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

If you remove the start or end Cross-Section and fail to replace them with a new cross-section vector then the preview will no longer show intermediate lines to that point on its length. This means the shape will start or stop at that cross section and not go all the way to the start/end of the line. You can either add a new cross section or drag an existing one to that position if you need to resolve this.

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

If this option is checked, ✓ then the tool will create a sharp corner in the Component where there are discontinuities in the drive rail vector. When unchecked the shape will be rounded as it goes around the discontinuity. Below you can see a rectangular drive curve with a simple cross section being extruded around it, the one on the left has the Create sharp corners option selected and the one on the right without.

Create sharp corners checked ✓

Create sharp corners un-checked

When checked ✓ this option will ensure that as the shape is extruded that it goes from a particular span/node in one cross section to the same span/node on the next cross section. For some applications this can give the user more control over the way the shape flows.

Using the above vector selection, the shape below left will be created with Sweep between spans checked ✓ and the shape on the right is created with the option un-checked. Note that on the left hand picture the crease in the shape goes from node to node in the cross sections as the spans flow exactly from one to the next. On the second picture the shape just linearly flows from one cross section to the next evenly with no additional control.

Sweep between spans checked ✓

Sweep between spans un-checked

As the extruded shape passes through each cross section the default is for it to flow smoothly through the profile. This can be edited by right-clicking over a cross section and unchecking the Smooth option. The middle node on the cross sections preview in the 2D View will be blue if it is smooth and white if it is un-smooth.

Using the above vector selection, the shape below left will be created with the Smooth option checked ✓ and the shape on the right is created with the option un-checked. Note that on the left hand picture the shape flows smoothly through each span, on the second it goes directly from cross section to cross section in a straight transition.

Smooth checked ✓ on all cross sections

Smooth un-checked on all cross sections