Cut Parameters: Raster
Use this page to configure the cutting passes for a Raster toolpath. Use this toolpath to create parallel finish passes with a constant stepover, aligned at an angle that you enter. This lets you optimize the direction of the cuts to your part geometry for the most efficient cuts.
| 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 your Reseller for more information. |
|
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. |
|
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. |
|
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. |
Cutting method
Orients the cutting direction. Select one of the following options:
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
- One Way: Cuts one direction, steps over to the next cut while making a rapid move to same start side of the cut, and cuts in the same direction as the previous pass.
- One Way: Starts with climb cutting and cuts each pass in the same direction.
- Other Way: Starts with conventional cutting and then cuts each pass in the same direction.
- Down Mill: Cuts in only the down direction.
- Up Mill: Cuts in only the up direction.
In some cases, it may not be possible to maintain a climb or conventional cut direction due to the nature of the toolpath motion. For example, the toolpath below starts from the outside and runs in a clockwise direction. The boss is climb cut, while the cavity is conventional cut.
Tip compensation
Select whether the compensation point will be the center of the tool or the tip. Compensating to the center of the tool is frequently used with ball cutters where compensation is applied at the control.
Optimize cut order
Keeps the tool within an area until all cuts in that area are completed.
| Optimize cut order off | Optimize cut order on |
|---|---|
|
|
Stepover
Places the tool in an area and keeps it there until all cuts in the area are made. This is a 2D value measured parallel to the tool plane.
Scallop height
Unavailable for tools with a corner radius equal to zero. Specifies the spacing between cutting passes in terms of the height of the scallop that is left. Mastercam will calculate the Stepover based on the value that you enter here and the selected tool.
The Stepover and Scallop height fields are linked so that when you type a value in one field, the other is automatically upated. This lets you specify the spacing between your cutting passes in terms of either the Stepover distance or the Scallop height. Scallop height is calculated against a flat surface. Bull nose tools produce no Scallop height unless the Stepover is large enough.
Machining angle
Orients the cutting passes. Select one of the following:
-
Custom: Select to manually enter the angle. When Custom is set to 0, the cutting passes are parallel to the X axis; at an angle of 90 they are parallel to the Y axis. Enter an intermediate angle to adjust the direction of the passes to specific part features or geometry for the most efficient machining action.
-
Automatic: Select to have Mastercam automatically set different angles to maximize the length of the cut pattern and/or minimize the connecting moves.
Perpendicular fill
Available when Machining angle is set to Custom. Select to limit raster passes relative to a cutoff distance of 1.4 times the Stepover. Perpendicular fill limits raster passes and then fills in the limited areas with perpendicular raster motion to create a clean result. Below is an example of a part with the Stepover set to 1.0.
| Perpendicular fill on | Perpendicular fill off |
|---|---|
|
|
Overlap (Down/up mill)
Enter a distance here to ensure that the toolpath does not leave unwanted scallops or cusps in the transition areas between passes of different direction.
Shallow angle (Down/up mill)
In areas where the Machining geometry is almost flat, there is no advantage to machining up or down. Mastercam creates either down or up milling passes. Enter the angle that defines the region where this can occur.





