Setup: FBM Mill
Use this page to define the tools Mastercam selects for the FBM Mill-generated toolpaths. FBM Mill locates features based on the Search plane you choose and the parameters you set in the Feature detection page.
You can optionally add toolpaths to the FBM Mill toolpath group
to rough and finish the outside profile of the part.
Tool selection can include any combination of the following sources:
- Up to 10 preferred tools that you define in each type of FBM Mill tools page.
- Tools in the Mastercam part file
- Tools in a specified tool library
- Tools that Mastercam creates as needed
Mastercam chooses tools from only the selected sources. Red lines connecting the tool source checkboxes show the hierarchical order in which Mastercam searches for tools.
| Example 1 | Example 2 | Example 3 |
|---|---|---|
|
|
|
|
Tool creation parameters in this page are available only when your tool selection includes Create as needed.
| 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. |
Automatic initial hole / feature detection
When selected, Mastercam automatically detects features when you choose the FBM operation. If you save the setting to your toolpath .mcam-defaults file and use that file in the active machine group, Mastercam automatically detects features every time you choose the FBM operation. Otherwise, this setting affects only the current Mastercam session when the current toolpath defaults file is used.
Detection analyzes the solid based on current FBM parameters and determines which features to include in the Features page (FBM Mill and FBM Drill). When you accept the FBM operation, Mastercam creates toolpaths for all features in the Features page list that can be machined . Note that options at the top of the dialog box allow you to save parameters to defaults file and reload parameters from defaults file. Select Detect in the FBM dialog box at any time to analyze the solid based on your current parameters, and to update the Features page.
Limit search to plane / Search plane
Detects only features that can be machined in the selected plane. You can choose from Mastercam's standard planes, or set the plane by selecting a face or geometry in the graphics window.
Group by (FBM Mill)
Controls the organization of FBM Mill-generated toolpaths in the Toolpaths Manager, including their subgroups, sequence, and the number of operations. For complex nested pockets, FBM Mill creates a separate zone for each Z depth. For each zone, FBM Mill generates a set of toolpaths to completely machine the zone including roughing, restmill, and finish toolpaths for walls and floors.
- Feature & Zone: Mastercam creates a separate subgroup in the Toolpaths Manager for each zone. Each subgroup contains a sequential list of the zone's FBM Mill-generated toolpaths.
- Minimize tool changes: After generating toolpaths based on the solid model's features and zones, Mastercam sorts the toolpaths into subgroups using the following hierarchical criteria: operation type (roughing, restmill, and finish), tool diameter (largest to smallest), sequence (chronologically by feature and zone), and restmill overlaps (restmill operations with smaller tools at higher Z depths are ordered before restmill or roughing operations at lower Z depths)
Tool selection (preferred tooling, part, library, create)
Select one or more of the following options to tell Mastercam where to locate tools for the FBM-generated toolpaths. The options display in the same hierarchical order Mastercam uses when searching for an appropriate tool. If an appropriate tool is not available in the first selected source in the hierarchy, Mastercam ends the search if no other tool selection options are activated. Otherwise, the search continues with the next selected source in the hierarchy.
- Preferred tooling (FBM Mill only): Searches the preferred tools list defined in the Facing tools, Roughing tools, Restmill tools, and Finish tools pages to find an appropriate tool for the operation. Mastercam searches the preferred tool list from the largest to smallest tool and stops at the first tool small enough to machine the feature (even if a more appropriate tool is available in another selected source). If only preferred tooling is selected but the preferred tools list is empty for the operation type, FBM cannot create the operation.
- Use tools in part file: Looks in the current Mastercam file for an appropriate tool. The tools do not have to be used in previous operations to be available to the FBM operation. Note that, when searching preferred tooling or tools in the part file, the Allow use of tool and Automatic tool selection settings in FBM Mill’s tool pages do not apply.
- Use tool library: Searches the selected tool library for the necessary tools.
- Create as needed: Creates the necessary tools using the tool creation parameters you define.
- For FBM Drill and Wizard Holes operations, the tools must match within the specified Diameter matching tolerance.
- To completely machine detected features and remove all material, Mastercam must have access to, or be allowed to create the necessary tools. Use the icons in the Features page list to verify each feature’s machining status.
Rough / Finish outside of the part
Select to add 2D roughing or finishing operations for cutting the solid model's outside profile. You can choose either or both operation types. You can skip the roughing contour and add only a finishing contour, if this strategy is best for your application.
Tool library
For FBM toolpaths, available only when Use tool library is selected in the FBM Drill or Wizard Holes Tools page, and the FBM Mill Setup page. Displays the tool library name where Mastercam selects tools for the toolpaths.
Comment
Enter comments for the toolpath. Comments help identify the operation in the Toolpaths Manager. These can be output in the NC file when you post if you select the proper option in the Files tab of the Machine Group Properties. Comments entered for FBM operations are copied to their generated toolpaths. For example, the same comment you enter for an FBM Drill operation appears in all of its generated drill cycles. This can help you maintain a relationship between FBM "parent" and "child" operations.
Tool creation (FBM Mill)
Available only when tool selection includes Create as needed. Mastercam uses the parameters you choose in this section to create new tools for FBM-generated toolpaths. Choose one of the following options to define what to do when the feature depth exceeds the tool length.
- Create one tool for all depths: Creates a single tool capable of meeting the longest depth requirement, based on detected features and FBM operation parameters.
- Create one tool for each depth: Creates and uses separate tools for each depth.
- Create tools in length increments of: Creates an incremental series of tools. Each new tool length is created as a percentage of the current tool. For example, if you enter 25%, Mastercam creates the next new tool 25% longer than the original tool.





