Feature Detection: FBM Mill
Use this page to control the types of features FBM Mill detects. For example, you can include pockets that extend through the part and set a minimum diameter to exclude small drill holes from detection.
You can choose a pocketing or hole milling strategy to machine the round features FBM Detects. If you choose Hole milling, use the parameters on the Hole Milling and the Circle Mill or Helix Bore pages to define the toolpath settings.
During feature detection, Mastercam creates edge curve geometry for the FBM Mill-generated toolpaths. Use options on this page to assign a level to this geometry.
Only features that match your detection criteria appear in the Features page for review. Mastercam automatically creates toolpaths for detected features when you save the FBM Mill operation.
Choose Detect (shown below) in this dialog box to detect features. You can also configure Mastercam to detect features when the FBM Mill dialog box opens. To do this, select Automatic initial feature detection in the Setup page, and then save the setting to the operations .mcam-defaults file.
| 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. |
Through features
Select to allow FBM Mill to detect and include pockets that extend through the whole model. Choose one of the following options to control how Mastercam cuts the through pockets. Then enter the corresponding value in the field.
- Stock to leave: Sets the amount of material to leave at the bottom of the stock. Use this option to protect what is underneath the part during the machining process.
- Additional break through: Sets the depth of the cut beyond the bottom of the part.
Edge curves
During feature detection, Mastercam creates the edge curve geometry that is required by the FBM-generated toolpaths to machine detected features. Choose one of the following options to tell Mastercam where to place this geometry. Note that the edge curve geometry is blanked; Use Unblank on the Home tab to view it.
- Place edge curves on level: Defines the level where the FBM-generated geometry is created.
- Place edge curves on first unused level greater than: Places the FBM-generated geometry on the first unused level it finds that is greater than the specified level.
Recognize holes greater than this diameter as features
Eliminates from detection any through holes that are not through pockets, for example, drilled holes. FBM Mill detects only through holes with a diameter that is greater than the value you enter in this field. All holes that are equal to or smaller than the entered diameter are excluded from detection.
Mill round features with this cycle
Choose one of the following strategies for machining the round hole features that FBM Mill detects in your solid model:
- Pocket: (default) Generates pocketing toolpaths for round hole features, allowing you to output separate rough, rest, and finish toolpaths.
- Hole milling: Generates a single Circle mill or Helix bore toolpath to machine round hole features. After choosing Hole milling, use the parameters on the Hole Milling, and the Circle Mill, or Helix Bore pages to define the toolpath settings.





