Tool Parameters: Automatic Arc Drilling
Use this tab to select the tools needed for automatically created drill operations. This tab is used by the Automatic drilling and Start Hole features. You can also modify tools for Solid Drill operations.
The Solid drill toolpath was removed from Mastercam. However, you can modify Solid drill operations that were created in prior versions of Mastercam, and regenerate their drilling cycles. Mastercam replaces the Solid drill toolpath type with FBM Drill, a more powerful and customizable solid drilling application.
Select checkboxes to activate other advanced toolpath setup options, such as home and reference positions, rotary axis parameters, etc.
Finish tool type
Determines what type of tool is used for the last drill operation to be created for the holes. Choose Drill, Tap RH Coarse, Tap RH Fine, Tap LH Coarse, Tap LH Fine, Reamer, Boring Bar, or End mill-Flat from the drop-down list. To determine which drill cycle will be used for the final operation, Mastercam uses the drill cycle stored with the tool you select here. If you select the flat end mill, the system uses a drill/counterbore cycle for the finish drill operation.
Create arcs on selected points
If you have selected points instead of arcs, create circles around the points by entering a diameter in the field. If you do not enter a diameter value, Mastercam will not create the holes.
Override geometry diameter
If you have selected arcs instead of points, select this option to machine a hole that is a different size than the arcs. This is especially useful for tapped holes. Since Mastercam chooses the tap size based on the diameter of the selected arcs, this can be a problem when the arcs are based on the minor diameter of the holes. After selecting this option, enter the desired diameter in the Circle diameter field.
Circle diameter
The desired diameter of the drilled holes, if different than the selected arcs.
Suppress "accept closest matching tool" prompts
Accepts all tools pulled from the tool library for the drill cycles. The tools must match within the diameter match tolerance.
None
Does not create a chamfer on the drill holes.
Add depth to spot drilling operation
Creates a chamfer on the drill holes as the final move in the spot drilling toolpath. Only available if you select the Generate spot drilling operation option.
Make separate operation
Creates a separate operation to cut the chamfer. This will appear in the Toolpaths Manager as a separate operation that you can edit independently.
Chamfer size
Sets the width and depth of the chamfer on the drill holes. Only available if you select Add depth to spot drilling operation or Make separate operation.
Generate spot drilling operation
Creates a spot drilling toolpath before any pre-drilling or finish drill cycles.
Maximum tool depth
Sets the final depth for the spot drill toolpath.
Default spot drill diameter
Sets the size of the tool used for the spot drilling toolpath. A spot drill of this diameter must exist in the tool library.
Select default spot drill
Opens the Tool Selection dialog box so you can select a spot drill.
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.
Home pos
Sets the position on the machine tool where the tool returns for tool changes and at the end of the NC program. The default home position is determined by the active machine and control definition; click this button to override it for this operation.
Reference point
A reference point is a location that the tool moves to between the home position and the start of the toolpath (approach point), and another location that the tool moves to at the end of the toolpath before returning to the home position (retract point). Select this option to use the currently programmed reference points, or click the button to set new reference points for this operation or to apply default reference points from the current machine definition or axis combination.
Mastercam Lathe lets you store separate reference points for ID and OD work. Mastercam will automatically select the proper ones.
Rotary axis
Sets parameters for rotary movement or axis substitution. This option is only available if your machine definition is configured to support rotary movement.
Planes
Click to set or change any of the following:
- the tool plane (Tplane) or work coordinate system used for the operation
- the Tplane or WCS origin
- the work offset associated with this operation.
For certain types of operations, you can also change the construction plane (Cplane).
Misc values
Select to set the values of custom integer and/or real variables that
have been defined for this machine. Click the button to review or change the values.





