Floor Finish: FBM Mill
Select Enable floor finish to add finish passes for the floor of each pocket feature in the FBM Mill operation. When this option is deselected, Mastercam creates only roughing and restmill operations for pocket floors. Finish toolpaths remove material left from the restmill operations to the Stock to leave depth you define in this page.
- 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. The exceptions are horizontal area passes in 2D high speed toolpaths, and 3D high speed toolpaths.
- Other parameters for the toolpath type come from values in the operations .default 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 floor finish
Select to add finishing operations for the detected feature's horizontal drive surfaces and to activate the parameters on this page. FBM Mill generates 2D High Speed Area Mill toolpaths with a From outside strategy to finish open pockets and an Area Mill strategy to finish closed pockets.
Cutting method
Use these options to orient the cutting direction. You can select either Climb milling or Conventional milling.
XY Stepover
Sets the spacing between passes in the X and Y axis for the FBM-generated toolpath type (Area Mill for open and closed pockets or Restmill). Mastercam computes the optimum spacing within the specified value. Choose one of the following options, and if necessary, enter the corresponding value.
- Use defaults: Uses the XY stepover defaults defined for the FBM-generated toolpath type either from the toolpath .mcam-defaults file. Or, from defaults in the tool definition if this option is enabled in the machine group's Tool settings tab.
- % of diameter: Calculates the XY stepover as a percentage of the tool diameter.
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.
Stock to leave on walls
Sets the amount of stock on selected vertical machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not vertical, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.
Stock to leave on floors
Sets the amount of stock on selected horizontal machining geometry. Enter a positive value if you do not want to remove all stock or enter a negative value to remove more stock. If the machining geometry (or a portion of it) is not horizontal, Mastercam interpolates a value between the Stock to leave on floors and Stock to leave on walls amounts.
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.





