Depth Cuts page: Pocket
Select Depth cuts to activate the options in this page, and to add the following features to a 2D Pocket toolpath:
- Divide the total pocket depth in increments. These will be used for both the roughing cuts and the finish passes on the walls.
- Create finishing passes for the floor of the pocket.
- Create tapered walls and islands.
In addition, you have the option of outputting subprograms for each depth. This option works only if the proper subprogram functionality has been enabled in your control definition.
To set the number of depth cuts, enter a maximum rough step. Mastercam divides the total depth into equal steps. Or, enter the exact number of finish steps and the size of each finish step. Mastercam never creates unequal rough depth cuts.
| 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. |
Maximum rough step
Sets 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. The value is calculated as a percentage of the tool diameter if you select Use tool's step, Peck, or Coolant option in your machine group properties.
Number of cuts (Finish)
Sets the number of finish cuts for the toolpath. This number multiplied by the finish step value equals the total amount of stock cut by the finish passes. Setting the number of finish cuts to 0 creates no finish cuts.
Step (Finish)
Sets the amount of material removed in the Z axis with each finish cut. This number multiplied by the number of finish passes equals the total amount of stock cut by the finish passes. The value is calculated as a percentage of the tool diameter if you select the Use tool's step, Peck, Coolant option in your machine group properties..
Override feed speed
Allows you to override the speed and feed values for finish passes, providing better control for floor finishing. Select one or both of the following options:
- Feed rate: Select to enter a different feed rate for the finish passes than the feed rate used for roughing. You may want to increase the feed rate because the tool usually cuts less material during finish passes.
- Spindle speed: Select to enter a different spindle speed for the finish passes than the spindle speed used for roughing. You may want to increase the spindle speed because the tool usually cuts less material during finish passes.
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.
Use island depths
When this option is selected, Mastercam passes the tool over the island until it reaches the depth of the island. It then goes around the island until it reaches the final depth. When this option is deselected (default), the toolpath goes around the island regardless of the island depth.
Subprogram
Sets values in the subprogram lines in the NCI file to indicate a section of the operation that is repeated at a different location (for example, a drill cycle or depth cut). This information is then passed to the post processor. The control definition must be set to support subprograms for this function to work.
In some instances, you might be able to select absolute or incremental subprograms. An absolute subprogram contains absolute coordinate values; in other words, the same points are machined every time the subprogram executes. With an incremental subprogram, the points which are machined are relative to the tool's location when the subprogram is called. Typically an absolute subprogram will have a G90 code while an incremental one will have a G91.
Depth cut direction
Sets the depth cut direction:
- Stepdown: Cuts from top to bottom.
- Stepup: Cuts from bottom to top.
Undercut (undercut tool only)
Select when using an undercut tool to support tool compensation.
Depth cut order
Determines the order of the depth cuts based on the selected option.
- By pocket: Performs all depth cuts in a region, contour, or pocket before moving to the next contour or region.
- By depth: Creates depth cuts at the same level in every contour or region and then descends to the next depth cut level. This option can be used for thin-walled parts using soft materials such as aluminum or graphite.
Tapered walls
Angles the depth cuts from the top of stock to the final depth. Not available if you use subprograms. Note that if you have chained the bottom of the pocket instead of the top, the upper cuts will be outside the chained geometry.
Taper angle
Sets a taper angle for the contour or pocket walls.
Island taper angle
Sets the taper angle for islands.





