Finishing: Pocket
Select Finish to activate the options in the Finishing page to create finishing passes for your pocket toolpath. Leave this option deselected to create only roughing passes. Follow these general guidelines to create finishing passes:
- Enter the number of passes.
- Define the amount of stock to remove with each pass.
- Select the type of cutter compensation.
You can also choose to override the feed rate and/or spindle speed that was set in the Tool page, and to divide the finish pass into multiple depth cuts for thin-wall pockets.
The entry method selected in the Entry Motion page applies only to roughing passes. For finish passes, Mastercam automatically places the starting point at the midpoint of the first chained entity in the chain direction. Use the Lead in/out page to create more refined entry and exit moves.
| 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. |
Finish
Use the options listed to create finish passes.
Passes
Enter the number of finish passes to create on the selected geometry. Entering 0 creates no finish passes.
Spacing
Enter the distance between finish passes.
Spring passes
Enter the number of spring passes for the toolpath. Spring passes create additional finish passes along the same path as the last finish pass. This can be used for parts with thin material that may have flexed away from the tool during previous passes.
Cutter 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.
Finish outer boundary
Creates a finish pass along the outer boundary.
Start finish pass at closest entity
When checked, begins the finish pass starting with the closest endpoint of the closest entity at the end of the roughing toolpath. When cleared, the finish pass begins with the first entity in the chain as it was originally selected.
Keep tool down
Determines whether or not to retract the tool between passes.
Even if Keep tool down is selected, other parameters, such as Entry method, may require the tool to retract.
Optimize cutter compensation in control
Eliminates arcs in the toolpath that are less than or equal to the radius of the tool and helps prevent gouging. This field is available only when Cutter compensation is set to Control and applies only to that setting.
Machine finish passes only at final depth
Select to perform the finish passes only at the final cutting depth. Deselect to perform finish passes at all depths. Note that this option applies to Pocket toolpaths, and 2D High Speed Peel Mill, Blend Mill, or Dynamic Contour toolpaths configured with multiple depth cuts.
Machine finish passes after roughing all pockets
Performs finish passes after all rough cuts and depth cuts have been completed.
Feed rate
Enter a different feed rate for the finish passes than the feed rate used for roughing. This lets you adjust the chip load for the finishing operation.
Spindle speed
Enter a different spindle speed for the finish passes than the spindle speed used for roughing. This lets you adjust the chip load for the finishing operation.
Thin wall
Enables finish passes for thin wall pockets. Only available when Machine finish passes only at final depth and Machine finish passes after roughing all pockets are deselected.
Z finish passes per rough depth cut
Sets the number of finish passes on thin wall pockets. The maximum stepdown from the Depth Cuts page is divided by this number to calculate the maximum stepdown for each finish pass. For example, if the maximum depth cut is 1.5 and you enter 2 in this field, the maximum finish stepdown is set to 0.75. Breaking the finish stepdown into multiple passes helps prevent breaking or over-stressing the thin walls.
Maximum calculated finish step
This is the step size Mastercam calculates by dividing the roughing step size by the number of finish passes entered in this page. You cannot edit this field here. Use the Depth Cuts page parameters to change the size of the finish step.
Maximum rough stepdown from depth cuts
The maximum amount of material removed in the Z axis with each rough cut. Mastercam calculates equal rough cuts no larger than the maximum rough step until it reaches the final Z depth. You cannot edit this field here. Use the Depth Cuts page parameters to change the size of the rough step.
Climb
Cuts in one direction with the tool rotating in the opposite direction of the tool motion. For face toolpaths that use Zigzag or One way cutting methods, Mastercam provides optional settings that reverse the direction of the final cutting pass for the toolpath. This strategy can prevent burring along the opposing edge of the face.
Conventional
Cuts in one direction with the tool rotating in the same direction as the tool motion. For face toolpaths that use Zigzag or One way cutting methods, Mastercam provides optional settings that reverse the direction of the final cutting pass for the toolpath. This strategy can prevent burring along the opposing edge of the face.





