Roughing: Pocket
Select Rough to activate the options in this page, and to create roughing passes for your pocket toolpath. Leave this option deselected if you want Mastercam to create only finish passes.
Then, select a cutting method from the large window. The parameters you can choose changes based on the selected cutting method. For example, choosing a High Speed cutting method activates the Trochoidal cuts parameters.
When you complete the parameters on this page, use the Entry Motion page to define ramp or helical entry moves for roughing passes.
| 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
Click on a cutting method to select it. Not all parameters listed in the Roughing page are available for every cutting method.
Stepover percentage
Sets the distance between cutting passes in the X and Y axes as a percentage of the tool diameter. Changing this value automatically adjusts the stepover distance.
Stepover distance
Measures the distance between cutting passes in the X and Y axes. This option calculates as a distance in the X and Y axes and equals the stepover percentage multiplied by the tool diameter.
Roughing angle
For pocket toolpaths, sets the angle that the tool moves at during the roughing passes for Zigzag and One Way cutting methods.
Minimize tool burial
Clears out areas around pocket islands to avoid tool damage due to burying the tool in too much stock. Applies to Zigzag, Spiral, Spiral Clean Corners and Constant Overlap pocket toolpaths.
Spiral inside to outside
Applies to all spiral pocket toolpaths. The toolpath spirals from the center (inside) to the wall (outer) of the pocket. If you do not select this option, the toolpath spirals from the outer wall of the pocket to the center.
Display stock for constant overlap spiral
Available for the constant overlap spiral roughing option. Previews the amount of stock removed by the roughing passes.
Tolerance for remachining and constant overlap spiral
Defines an additional tolerance value which Mastercam uses for remachining pocket toolpaths or constant overlap spiral pocket toolpaths. The accuracy of these pocket toolpaths is controlled by this tolerance. Smaller tolerances increase accuracy but can result in longer processing times. You can specify the tolerance as a percentage of the tool diameter or as an absolute value. If you type a value in one field, the other automatically recalculates.
Off
Turns off trochoidal cuts. Mastercam inserts loops only at the stepover of each cut of the toolpath.
Full material only
Inserts arcs (loops) only when the tool is buried in the material more than the stepover amount. The tool moves along the loops until it becomes less buried, then returns to a cutting path without loops.
Entire pocket
Inserts arcs (loops) throughout the entire toolpath. Use when the stepover or stepdown is very large.
Loop radius
Sets the radius used in high speed loop motion.
Loop spacing
Sets the stepover between successive high speed loops.
Corner smoothing radius
Allows the tool to move in an arc when changing direction around a corner. Creates smooth continuous motion instead of stopping the tool between changes in direction.





