Cut Parameters: Area Roughing
Use this page to configure the cutting parameters for an Area Roughing toolpath. The toolpath creates multiple passes at different Z heights, and multiple profiles at each Z height.
| 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. |
Closed contour direction
Orients the cutting direction of the closed contours. Closed contours contain continuous motion without a need for a retract or reversal of direction. Select one of the following options:
- Climb: Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
- Conventional: Cuts in one direction with the tool rotating in the same direction as the tool motion.
Open contour direction
Orients the cutting direction of the open contours. Select one of the following options:
- One Way: Cuts the open contour by taking a pass, moving up to the retract height, moving back to the beginning of the cut, and taking another pass in the same direction. All passes are in the same direction.
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
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 |
|---|---|
|
|
Stepdown
Determines the Z spacing between adjacent cutting passes.
Add cuts
Adds cuts at shallow areas of the profile so that the toolpath does not have excessively large horizontal spacing between cutting passes.
Minimum stepdown
Sets the minimum distance between the added Z cuts in the shallow areas of the part.
Maximum profile stepover
Determines the maximum change in the surface profiles for two adjacent cutting passes. This represents the maximum value of the shortest horizontal distance between adjacent points on the two profiles.
For most applications, the Maximum profile stepover should be greater than the Stepdown. Otherwise, toolpath calculation time can increase significantly. If you think that your toolpath is taking too long to calculate, check to make sure that the Maximum profile stepover is greater than the Stepdown.
Corner rounding
Activates toolpath corner rounding, which replaces sharp corners with arcs for faster and smoother transitions in tool direction. Once you activate corner rounding, set the maximum radius, profile tolerance, and offset tolerance.
- Maximum radius: Enter the radius of the largest arc that you will allow Mastercam to insert to replace a corner. Larger arcs result in a smoother toolpath, but with greater deviation from the originally programmed toolpath.
- Profile tolerance: Represents the maximum distance that the outermost profile of a toolpath created with corner rounding can deviate from the original toolpath.
- Offset tolerance: Represents the maximum distance that a profile of a toolpath created with corner rounding can deviate from the original toolpath. This is the same measurement as the profile tolerance but is applied to all the profiles except the outermost one. This lets you maintain different tolerances for the first profile and subsequent profiles.
Percentage of diameter (XY stepover)
Expresses the maximum XY stepover as a percentage of the tool diameter. The Maximum (XY stepover) field will update automatically when you enter a value in this field. The actual stepover is caFlculated by Mastercam between the Minimum and Maximum values.
Minimum (XY stepover)
Enter the smallest acceptable distance that you want Mastercam to use for a stepover distance between two cutting passes. Mastercam will calculate an XY stepover that lies between the minimum and maximum values that you enter here.
If you are using Corner rounding, make sure that the Minimum stepover is greater than the Offset tolerance value and less than the radius of the tool shaft.
Maximum (XY stepover)
Enter the largest acceptable distance that you want Mastercam to use for a stepover distance between two cutting passes. Mastercam will calculate an XY stepover that lies between the minimum and maximum values that you enter here.
This field is linked to Percent of diameter, so that you can express the maximum stepover as either an absolute distance or as a percentage of the tool diameter. When you make an entry in one field, the other automatically updates. The default maximum stepover is 45% of the tool diameter. Ensure that the maximum stepover is at least twice as large as the minimum stepover.





