Roughing: FBM Mill
Select Enable roughing on this page to add roughing toolpaths to the FBM Mill operation and to define their cutting passes. In the FBM Mill toolpath group, Mastercam creates the roughing toolpaths before any restmill or finish passes.
For complex nested pockets, Mastercam creates a separate zone for each depth and creates the edge curve geometry required to machine it. Roughing is the first series of operations for each pocket zone. A single pocket with multiple zones will have multiple roughing operations. Mastercam uses 2D high speed toolpaths, such as Area Mill, to efficiently rough pockets.
- Mastercam selects tools for rough 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.
- If you edit the Entry method options, they will not be updated if you re-chain.
| 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. |
Cutting method (FBM)
- 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 the approach distance, which you define as a percentage of the tool diameter.
Entry method
Defines the entry point and cutting strategy used to create the toolpath. Choose one of the following options:
- Helix only: The tool helixes into the pocket and the dynamic pocketing cutting starts right away. This cutting strategy uses a dynamic milling motion growing outward from the entry motion. The helix is centered on the deepest point in the pocket, unless overridden (see Center helix on point).
- Helix followed by full medial burial: After the helix entry, the tool is fully buried as it moves along the medial axis (central spine of the pocket). Its purpose is to clear a slot for the subsequent passes so that they are not fully buried.
- Helix followed by trochoidal medial: The tool enters the pocket with a helix, and then moves along the medial axis (central spine of the pocket) with a trochoidal cut rather than a fully buried cut. This clears a slightly wider slot than full medial burial for the subsequent passes to be optimally engaged. This strategy avoids burying the cutter but takes longer.
- Profile: Creates a “follow boundary” ramp entry based on the shape of the offset pocket. The slot is cleared by taking lighter cuts in the Z axis. Subsequent cuts are properly engaged at the full cut depth.
- Medial: Creates a ramp entry based on the shape of the medial axis (central spine of the pocket). The slot is cleared by taking lighter cuts in the Z axis. Subsequent cuts are properly engaged at the full cut depth.
Profile ramp
Select to create a ramp motion to the next level. Instead of a simple straight line, the tool will track around the contour of the profile as it moves down to the next level.
Helical entry
Creates a helix at the center of the circle to begin the roughing motion. If off, the tool plunges to start the toolpath.
Output 3D arc moves
Select to output entry arc moves as 3D arcs, reducing the amount of NCI data created. Deselect to convert entry arcs to line segment output.
XY Stepover (FBM)
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 (FBM)
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 (FBM)
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 (FBM)
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 (FBM)
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.
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 on walls
Enter a value here if you do not want to remove all the stock from vertical drive geometry, such as surfaces, faces, or chains. If the drive 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. Note that, stock to leave on walls must be greater than or equal to the stock left on the floor. The exceptions are all 2D high speed toolpaths, and the 3D high speed horizontal area passes. For high speed horizontal area toolpaths, the wall geometry must be selected as drive geometry in order for the Stock to leave amount to be applied.
Stock to leave on floors
Enter a value here if you do not want to remove all the stock from horizontal drive geometry, such as surfaces, faces, or chains. If the drive 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. Note that, stock to leave on walls must be greater than or equal to the stock left on the floor. The exceptions are all 2D high speed toolpaths, and the 3D high speed horizontal area passes.
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.





