Wall Finish: FBM Mill
Select Enable wall finish on this page to add finish passes for the walls of each pocket feature included in the FBM Mill operation. When this option is deselected, Mastercam creates only roughing and restmill operations for pocket walls. There are the following restrictions for tapered walls:
- Positive angle only (no undercuts)
- Consistent linear angle for connected walls
- All boss angles within a feature will be cut with the smallest taper angle
- Draft faces must be tangential to internal corner fillets
- Mastercam selects tools for finish operations based on settings you choose in the FBM Mill Setup and Finish tools pages.
- Stock to leave on walls must be greater than or equal to the stock left on the floor.
- Other parameters for the toolpath type come from values in the operation's .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 wall finish
Select to add finishing operations for the detected feature's vertical drive surfaces and to activate the parameters on this page. FBM Mill generates 2D pocket toolpaths to finish internal feature walls and 2D contour toolpaths to finish external walls. Mastercam uses the remaining stock from the Restmill stock to leave to calculate the number of finish passes based on your settings.
Cutting method
Use these options to orient the cutting direction. You can select either climb milling or conventional milling.
Use defaults (Finish passes)
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.
Percentage
Calculates the stepover using the percentage of the finish tool diameter you specify. Mastercam calculates the number of finish passes based on the stepover you define and the remaining stock specified as the restmill stock to leave.
Number
Enter the number of wall finish passes. Mastercam calculates the stepover required to take the part from the restmill stock to leave to the finish stock to leave settings in the specified number of passes.
Spring passes
Creates additional finish passes along the same path as the last finish pass. In other words, use this option to create additional finish passes with a spacing of 0 between the passes. Can be used for parts with thin material that may have flexed away from the tool during previous passes. Enter the number of additional passes.
Overlap percentage
Sets the amount that the facing tool motion overlaps the outer boundary of the stock or the islands. This option cleans the edges of the faces and represents a percentage of the tool diameter. This field automatically calculates the overlap amount.
Cutter compensation
Choose Computerto use compensation in the computer, Control to use compensation at the machine tool, or Wear to use compensation at both places. Reverse Wear works just like Wear except that the wear adjustment is entered as a positive number.
Entry / Exit moves
Use these fields to define the tool moves Mastercam uses when entering and exiting finish cut passes. Your entry / exit move can include both lines and arcs. Enter arc or line dimensions as a percentage of the tool diameter. To use an arc only, enter a line length of 0. To use a line only, enter an arc radius of 0.
Perpendicular
Rotates entry or exit lines 90 degrees towards the cutter compensation direction.
Tangent
Select to extend the open chain selected for the machining region tangentially to the stock.
Line Length
Sets the line length for entry or exit lines. Enter a percentage of the tool diameter or an exact length. Mastercam automatically updates the other field when you enter a value in one of them. Set to 0 if you just want an entry arc and do not want an entry line.
Arc Radius
Defines the entry or exit arc's radius. The arc is always tangent to the toolpath. Enter a percentage of the tool diameter or an exact length. Set to 0 if you just want an entry line and do not want an entry arc.
Sweep angle
Sets the sweep angle of the entry or exit arc.
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 (Depth cuts)
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.
% Long tool
Reduces the stress on long tools by using separate depth cuts or an XY stepover calculation for them. Long tools are defined by the length to diameter ratio you define in the L/D field.
- For depth cuts, Mastercam multiplies the diameter of the tool by the diameter percentage you enter to determine the maximum depth and number of cuts made with long tools in the FBM-generated toolpath.
- For XY stepover, Mastercam calculates the XY stepover as a percentage of the tool diameter you enter.
# of cuts
Enter the number of passes you want Mastercam to create in the FBM-generated toolpath.
Tapered wall stepdown
Set the stepdown value to be used on tapered walls. Recognize tapered features must be checked on the Setup page for the stepdown to cut a taper.
Stock to leave in XY
Determines how much stock remains in the XY direction when the operation is finished. Typically, this would be removed by a separate finish operation.
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.
Use long tool values when the length to diameter ratio is greater than (L/D)
Defines long tools using the length to diameter ratio you enter. When long tools are used for FBM-generated toolpaths, Mastercam applies the % Long tool values you set in the XY stepover and Depth cuts fields for roughing, restmill, floor finish, and wall finish cut parameters.





