Facing: FBM Mill
Select Enable facing on this page to add a face toolpath to the FBM Mill operation and to define its cutting passes. In the FBM Mill toolpath group, Mastercam creates the face toolpath first.
- Mastercam selects tools for face operations based on settings you choose in the FBM Mill setup and FBM Mill tools pages.
- Other parameters for the toolpath type come from values in the operations DEFAULTS file, as defined in the Files tab for the machine group. You can also use options in the machine group's Tool settings tab to replace some of the operation defaults with tool definition defaults.
| 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. |
Enable facing
Select to add a facing operation to the FBM-generated toolpaths and activate the parameters on this page. Mastercam adds the facing operation as the first toolpath in the FBM operation's toolpath group. The facing operation removes the material between the top of the stock and the part's highest geometry in the Z axis. Note that, although you select this option, Mastercam adds the face toolpath only if the stock height is greater than the top of the part geometry in the Z axis.
Stock to leave in Z
Determines how much stock remains in the Z direction when the operation is finished. Typically, this would be removed by a separate finish operation.
Depth cuts
Defines how Mastercam divides the total depth for the FBM-generated toolpath type into multiple depth cuts. Select one of the options, and if necessary, enter a value in the corresponding field.
Use defaults
Uses default parameters for this setting, either from values in the FBM-generated operation's .mcam-defaults file, as defined in the Files tab for the machine group, or from the tool definition when this option is enabled in the machine group's Tool settings tab.
% of diameter
Determines the maximum depth and number of cuts made in the FBM-generated toolpath by multiplying the diameter of the tool by the diameter percentage you enter in this field. For example, if you enter 10%, a 2 inch tool takes .02 passes.
# of rough cuts
Enter the number of roughing passes you want Mastercam to create in the FBM-generated toolpath.
Maximum cut depth
Sets the lowest point that the tool descends in the Z axis while cutting material in the FBM-generated toolpath.
Finish passes
Define the number of finish passes for the FBM-generated toolpath, and how much material is removed with each finish pass. If you enter 0, the roughing passes cut to the final stock to leave depth you defined in the Floor finish and Wall finish cut parameters pages.
Climb / Conventional (finish pass)
Select the cutting method from the drop-down list.
- 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.
Cutting method
- Zigzag: Moves the tool back and forth across the part.
- One way: Takes a pass with the tool, rapids up, moves back to the beginning of the cut, and takes another pass in the same direction. All passes are made in the same direction.
- Dynamic: Cuts from the inside out in a smooth controlled motion, maintaining a constant load on the tool with minimal entries and exits. When you choose this cutting method. Mastercam internally manages additional cut parameters (they appear unavailable for selection) with the exception of Approach distance, which you define as a percentage of the tool diameter.
Maximum stepover %
Sets the distance between adjacent passes in the FBM-generated toolpath. Enter the maximum stepover as a percentage of the tool diameter. Note that a smaller maximum stepover value may take longer to generate the toolpath.
Across overlap %
Sets the amount that the tool overlaps the stock perpendicular to the cut angle. Enter the across overlap as a percentage of the tool diameter.
Along overlap %
Sets the amount that the tool overlaps the stock parallel to the cut angle. Enter the along overlap as a percentage of the tool diameter. This value must be greater than or equal to the across overlap.
Approach distance %
Adds an additional distance to the beginning of the first cut. Enter the approach distance as a percentage of the tool diameter.
Exit distance %
Adds an additional distance to the end of the last cut. Enter the exit distance as
a percentage of the tool diameter.





