Circle Mill: FBM
Use this page to define circle mill roughing and finishing passes and set toolpath parameters for stock to leave, depth cuts, and entry/exit motion. You also configure the cutting method and the type of cutter compensation Mastercam uses for your FBM-generated circle mill 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. |
Single pass circle mil
Select to deactivate the Rough and Finish parameters on the page. When selected, FBM generates only single pass Circle mill toolpaths for the hole milling features it detects. Deselect this checkbox to create multiple rough and finish passes in the FBM-generated Circle mill toolpaths.
Disable pre-drilling
Available only for FBM Drill and Wizard Holes operations. Select to ignore the settings on the Pre-Drilling page, and exclude pilot hole drill cycles for features included in FBM-generated Circle mill or Helix bore toolpaths. Deselect to allow FBM Drill or Wizard Holes to consider pre-drilling parameters. If pre-drilling is active for the FBM operation, pre-drilling cycles are generated in addition to Circle mill or Helix bore toolpaths for hole milling features.
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.
Finish passes (FBM)
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.
Final depth
Performs finish passes only at the final depth.
All depths
Performs finish passes at every cut depth.
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.
Cutting method
Use these options to orient the cutting direction. You can select either Climb milling or Conventional milling.
Compensation
Choose how you want to handle cutter compensation:
- Computer: Mastercam computes the compensated toolpath and does not output control codes for compensation.
- Control: Mastercam outputs control codes for compensation and does not compute the compensated toolpath.
- Wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are the same.
- Reverse wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are opposite.
- Off: Mastercam programs the tool tip directly on the chained geometry and does not output compensation codes.
The options that are available to you are determined by the active control definition.
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.
Keep tool down
Determines whether or not to retract between depth cuts. Mastercam ignores this setting if the ramp entry option is used.
Start angle
Sets the angle where the helix bore toolpath begins.
Entry/exit arc sweep
Sets the included angle of each entry and exit arc. If the entry/exit arc sweep is less than 180 degrees, the system applies an entry/exit line.
Start at center
Begins the thread toolpath at the center of the selected arc. Only applies to ID threads.
Perpendicular entry
Enters the toolpath perpendicular to the first tool move.
Overlap
Sets how far the tool goes past the end of the toolpath before exiting for a cleaner finish.
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.
Minimum radius
Determines the smallest possible radius for the entry helix. Enter the minimum radius as a percentage of the tool diameter or as an absolute distance. Note that the absolute distance field is unavailable when defining FBM-generated toolpaths.
Maximum radius
Determines the largest possible radius for the entry helix. Enter the maximum radius as a percentage of the tool diameter or as an absolute distance. Note that the absolute distance field is unavailable when defining FBM-generated toolpaths.
Output 3D arc entry motion
Writes the entry helix to the NCI file as arcs. Using this option can create shorter NC files. If you turn off this option, the helix breaks into linear segments in the NCI file.
Tolerance
Controls the accuracy of the entry helix when broken into linear segments. A lower tolerance value produces a more exact entry helix, but may create larger NC files and take longer to process. Not available if you select Output arc moves.
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.





