Multi Passes: Contour, Model Chamfer
Activate this page by selecting Multi passes. When you define multiple cutting passes, the tool approaches the part geometry at the cutting depth in steps instead of cutting right to the part geometry.
- Rough passes, where Number is set to 4 and Spacing is set to 0.1.
- Finish passes, where Number is set to 2 and Spacing is set to 0.05.
Use the following guidelines to create roughing and finishing passes:
- Enter a value for the Number of passes.
- Define the Spacing distance.
- Set the machining depth for finish passes.
You can also combine multiple passes, which divide the distances in the XY or cutting plane, with depth cuts, which divide plunge moves into Z-axis increments.
Not all options are available for all toolpaths.
| 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. |
Number
Enter the number of cutting passes you want Mastercam to create.
Spacing
Enter the amount of stock to remove with each cut.
Spring passes
Enter the number of spring passes for the toolpath. Spring passes create additional finish passes along the same path as the last finish pass. This can be used for parts with thin material that may have flexed away from the tool during previous passes.
Apply to all finish passes
Select to apply spring passes after the last finish pass for each defined depth set by the Finish passes parameter. When deselected, spring passes are only applied after the last finish pass at the final depth.
Feed rate
Select to enter a different feed rate for the finish passes than the feed rate used for roughing. You may want to increase the feed rate because the tool usually cuts less material during finish passes.
Spindle speed
Select to enter a different spindle speed for the finish passes than the spindle speed used for roughing. You may want to increase the spindle speed because the tool usually cuts less material during finish passes.
Finish passes
- Final depth: Performs finish passes only at the final depth.
- All depths: Performs finish passes at every cut depth.
- Defined by rough depth cuts: Performs finish passes based on the number of rough depth cuts.
- Add between: Adds the specified number of finish passes between each depth cut.
- Per number of: Adds a finish pass at the specified interval of rough depth cuts. A multi pass finish is always added to the last depth cut.
Multi pass order
- By contour: Completes all multi passes in a chain before moving to the next chain.
- By pass: Orders the multi passes by pass number and completes the first pass on all contours before performing the next set of passes.
Rough pass cut direction
- One way: Maintains one cut direction for the multi pass cuts.
-
Zigzag: Alternates the multi pass cut direction between climb and conventional. This is supported only by open chains.
NOTEBoth options respect Keep tool down.
Keep tool down
Determines whether or not to retract the tool between passes.
When selected for Contour Remachining toolpaths, the tool moves between remachining passes are not gouge checked. Take the necessary precautions to eliminate the risk of gouging. Additionally, when selecting this option for an open Contour toolpath, use caution because the tool does not retract when moving from the end point to the start point of the toolpath and may result in a gouge.
Even if Keep tool down is selected, other parameters, such as Entry method, may require the tool to retract.
Machine finish passes after roughing all contours
Performs finish passes after all rough cuts and depth cuts have been completed.
Machine spring passes after finishing all contours
Performs spring passes after all finish cuts and depth cuts have been completed.





