Cut Parameters: Pocket
Use this page to enter cutting parameters and compensation options for a pocket toolpath. Selecting a Pocket type other than Standard activates additional parameters that display directly below the field. Use these fields to fine-tune the cutting action. The pocket type you choose is generally based on the pocket geometry.
| 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. |
Machining direction
Sets the machining direction of the toolpath. Select one of the following:
- Climb: Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
- Conventional: Cuts in one direction with the tool rotating in the same direction as the tool motion.
Tip compensation
Select whether the compensation point will be the center of the tool or the tip. Compensating to the center of the tool is frequently used with ball cutters where compensation is applied at the control.
Roll cutter around corners
Inserts arc moves around corners in the toolpath. Select None to guarantee all sharp corners, Sharp to only roll the tool around sharp corners (135 degrees or less), or All to roll the tool around all corners and create smooth tool movement. The radius of the arc moves equals the radius of the tool.
Linearization tolerance
Used when converting helixes from curves to lines. Smaller tolerance values make more accurate toolpaths, but may take longer to generate and create a longer NC program.
Create additional finish operation
Adds a finish operation to the Toolpaths Manager after the Pocket operation. The new finish operation uses the same parameters and geometry as the original Pocket toolpath, but consists only of finish passes. This allows you to select a different tool for the pocket finish passes. Generally, if you use this option, you specify the leftover stock amount in the Stock to leave on walls or Stock to leave on floors fields.
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.
Maintain sharp corners
Available only when a positive Stock to leave on walls value is entered. Rolls your tool around sharp corners while including the stock amount. The following images display how selecting this option affects your toolpath:
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.0.
-
Maintain sharp corners is not selected.
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.175.
-
Maintain sharp corners is not selected.
- Roll cutter around corners set to Sharp.
- Stock to leave on walls set to 0.175.
-
Maintain sharp corners is selected.
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.
Pocket type
Defines the type of pocket toolpath Mastercam creates. Note that, when you select a pocket type other than Standard, Mastercam displays additional parameters below the field. Use these parameters to fine-tune the cutting action. Choose from the following options:
- Standard: Use with only closed chains. Mastercam intelligently analyzes all selected chains and considers the largest of the closed chains to be the stock to machine. The tool is constrained by the machined area (the largest closed boundary selected). All other smaller closed chains within the largest chain are considered non-machinable areas and are avoided.
- Facing or Island facing: Use with only closed chains. Creates a pocket facing or island facing toolpath. Define the distance the tool can overlap the stock, and set an approach and exit distance to extend the toolpath with additional linear moves. For island facing toolpaths, you can also specify an amount of stock to leave on the tops of the islands.
- Remachining: Use with only closed chains. Calculates areas where the pocket roughing tool could not machine the stock and creates a second remachining pocket toolpath to clear the remaining material. Select the source of the operation that you are remachining and set a clearance amount. Then choose whether to add entry/exit moves to only rough passes, and whether to apply finish passes to the entire part (not just the remachined portion). You can also choose to display the stock left after remachining.
- Open: Can be used with open and closed chains. The distance between the start and end points of open chains is calculated and treated as closed geometry. Mastercam automatically enters and exits the pocket through the opening. When you choose Open pocket cutting method, Mastercam starts the toolpath at the open end of the pocket and cuts from the inside to the outside.
If Pocket type is set to Facing or Island facing, the following parameters display.
Overlap percentage
Sets the amount that the facing tool motion overlaps the outer boundary of the stock or the islands. This option cleans the edges of the faces and represents a percentage of the tool diameter. This field automatically calculates the overlap amount.
Overlap amount
Sets the amount that the facing tool motion overlaps the outer boundary of the stock or the islands. This option cleans the edges of the faces and calculates as a distance in the XY axis. This field equals the overlap percentage multiplied by the tool diameter.
Approach distance
Adds an additional distance to the beginning of the first cut. Enter the distance as a percentage of the tool diameter or as an absolute distance. Use the drop-down to select the location of the approach.
Exit distance
Adds an additional distance to the end of the last cut. Enter the exit distance as a percentage of the tool diameter or as an absolute distance.
Stock above islands
Sets the Z height above the islands where the facing should stop. This option leaves stock on the top of the islands for later machining.
If Pocket type is set to Remachining, the following parameters display.
Previous operations
Determines remaining stock for remachining by calculating stock removed during all previous contour, pocket, circle mill, and facing operations in the Toolpaths Manager.
The previous operation
Determines remaining stock for remachining by calculating stock removed during the previous contour, pocket, circle mill, or facing operation in the Toolpaths Manager.
Roughing tool diameter
Calculates the remaining stock based on the diameter and corner radius of a tool. Use this method to finish a toolpath without a previous operation.
- Roughing tool diameter: Enter the roughing tool diameter.
Clearance
Extends the toolpath at the beginning and end to prevent cusps of material from being left behind. Enter the clearance as a percentage of the tool diameter or as an absolute value.
Apply entry/exit curves to rough passes
When selected, Mastercam uses the values in the Lead In/Out page for roughing passes in the pocket remachining toolpath. (The Lead In/Out page is located under the Finishing page.) You do not need to enable parameters on the Finishing page to apply entry and exit curves to roughing passes. However, you must enable the Roughing page and define their settings. Then set entry and exit options for the roughing passes in the Lead In/Out page.
Machine complete finish passes
Creates finish passes over the entire part, not just the areas with remaining stock.
Display stock
Previews how much stock is removed during the roughing toolpath and the remachining or finishing toolpath, and how much stock is left after remachining.
If Pocket type is set to Open, the following parameters display.
Overlap
Enter either an absolute distance or a percentage of the tool diameter to set the distance by which the tool will overlap an imaginary line drawn across the open edge of the pocket (open chains). The dotted white lines in the following picture outline the applied overlap distance.
For closed chains, the overlap is applied to the largest closed boundary (machinable area) except where it is coincident with other chained geometry, as shown in the following picture. Note that, if you select Use Standard pocket for closed pockets, Mastercam does not apply the specified overlap to closed contours that are machined by the open pocket toolpath.
Use open pocket cutting method
This option applies to only open chains selected for the Open pocket toolpath. You can chain a combination of open and closed chains before selecting the Open Pocket type from the list on the Cut parameters page.
- Select to start the toolpath at the open end of the pocket and cut inside to outside. If you select this cutting method, the cutting method you choose on the Cut parameters page applies to only closed chains that were also selected for the pocket toolpath.
- Deselect this option to choose a different cutting method on the Roughing page. Mastercam applies the method you choose there to all chains (open and closed) selected for the open pocket toolpath.
The open pocket cutting method is best used for simple open pockets. If your open pocket has complex geometry, consider leaving this option deselected and use the Roughing page. to select a different cutting method.
Use Standard pocket for closed pockets
This option applies to only closed chains selected for the Open pocket toolpath. (You can select a combination of open and closed chains before choosing the Open Pocket type from the list on the Cut parameters page.) When creating a pocket toolpath, Mastercam intelligently analyzes all selected chains and considers the largest of the closed chains to be the stock to machine. All other smaller closed chains within the largest chain are considered non-machinable areas and are avoided, as shown in the following pictures.
-
Deselect this option (default) to allow Mastercam to apply the overlap percentage / distance that you define to the boundary of the machined area (the largest closed boundary selected).
-
Select this option to apply Mastercam's standard pocket cutting strategy; the smaller closed contours are avoided, but the tool is constrained by the machined area (the largest closed boundary selected) and no overlap is applied.





