Project Curves Options Page
Use the Project Curves Options page to set options for projecting a toolpath onto surfaces. You can choose from four strategies: User defined, Radial, Spiral, and Offset. Click the following Parameters link to see strategy definitions and option descriptions.
Parameters
Common toolpath dialog box controls
| Icon | Name | Description |
|---|---|---|
|
Detect (FBM Drill) | Analyzes the solid model and detects features based on the Feature Based Machining (FBM) operation's current parameters. View the results of all detected features and their machining information in the Features page. For more information, please refer to Detection States and Modes in FBM. |
|
Reselection is not available |
Hole Wizard features for a Wizard Holes operation can only be selected in Mastercam for SOLIDWORKS. Contact Mastercam for more information. NOTE
Mastercam for SOLIDWORKS is no longer supported starting with Mastercam 2024. |
|
Preview toolpath operations (FBM Drill/Wizard Holes) | Opens the Toolpath Operations Preview dialog box where you can view the list of operations FBM will generate using the current Features page list. |
|
Select default formulae file (3D high speed toolpaths) | Lets you select a different *.formula file, which Mastercam uses to calculate default values. |
|
Save parameters to defaults file | Makes the current toolpath settings the default for future toolpaths of this type. Saves the current values in the toolpath properties pages to the .mcam-defaults file specified in the machine group properties. |
|
Reload parameters from defaults file | Overwrites the current values in the toolpath properties pages with the toolpath's default parameters. These parameters are reloaded from the .mcam-defaults file specified in the machine group properties. |
|
Display graphical elements | Enables the display of graphical elements, such as plane labels and geometry colors. In 2D or 3D toolpaths Mastercam also has Display only elements on current page, Display plane labels, and Simplify plane display as options. |
|
Hide dialog | Minimizes the dialog box so that you can use other Mastercam functions, like changing your shading settings or the graphics window view. When finished, press [Esc] to maximize the dialog box. |
|
Tool Manager | Opens the Tool Manager. Use the Tool Manager to create and edit tool definitions and to work with tool libraries. When you close the Tool Manager, the toolpath dialog box will reappear just as you left it. |
|
Feed speed calculator | Opens the Feed & Speed Calculator dialog box where you can modify the calculated feed rate or spindle speed by adjusting the material and tool parameters. |
|
None |
Page window | This window displays all of the pages that are available to you, depending on the selected toolpath type. A green check mark indicates pages where data has changed in the current session. |
| None | Quick View Settings | This window summarizes key toolpath information from the Tool page, Coolant page, and Planes page. It updates automatically as you make changes to the different pages and is always visible. |
| None | Generate toolpath | When selected, automatically generates the toolpath when you click OK. For more information, refer to Accepting and Generating Toolpaths. |
|
OK | Generates the toolpath and closes the dialog box. If editing a toolpath, applies the changes and closes the dialog box. |
|
Apply | Applies your changes to the toolpath without closing the dialog box. |
|
Cancel | Closes the dialog box and cancels the toolpath creation. If editing a toolpath, any changes to the toolpath are discarded. |
Type
Generally, use the following strategies as finish operations.
-
User defined: Mastercam projects the curve you select onto the drive surfaces.
-
Radial: Mastercam projects a radial pattern with a constant pitch onto the surface. You define the center point for the radial pattern. Define the area with the start and end radius. You can also limit the area by an angular span between 0 and 360.
-
Spiral: Mastercam projects a spiral pattern with a constant pitch onto the surface. You define a center point for the radial pattern and define the area with the start and end radius. Machining starts from the inner circle, defined by the start radius, and cutting spirally in the outward direction, with a constant stepover in the 2D plane.
-
Offset: To finish complex shapes, use this strategy to create a 2D offset pattern that is based on a user-defined curve that is projected onto the surfaces. This machining strategy is effective on shallow areas. Defined curves can be an open or closed drive curve, and the offsets are parallel to the drive curve. Mastercam detects closed or open segments in the drive curve.
Projection dir.
Specifies the direction toward which the curves should be projected.
Center point
Specifies the radial pattern's center point. You can specify the center point, or it can be automatically detected.
Radius
-
Start: Specifies the radial area's start radius.
-
End: Specifies the radial area's end radius. You can set this yourself or have it generated automatically.
Angle
-
Start: Specifies the starting angle of the radial or spiral area.
-
End: Specifies the ending angle of the radial or spiral area.
Step direction
-
Left: Mastercam computes the toolpath inside the closed containment.
-
Right: Mastercam computes the toolpath outside the closed containment.
-
Both: Mastercam computes the toolpath both inside and outside the closed containment.
Cutting side
The cutting side can be left, right or center, depending on the cutting direction. Mastercam determines the cutting direction from the drive curve's chaining. The toolpath always starts with the chaining start point.
Number of cuts (left)
Specifies the number of cuts to generate. A value of 0 creates as many cuts as possible. Non-zero numbers define the exact number of cuts to generate.
