Cut Pattern: 3+2 Automatic Roughing
Use the options on this page to define and organize the cutting passes for your toolpath. Mastercam creates a series of 2D cutting passes in each cutting plane.
- Begin by selecting the cutting pattern from the Type drop-down. This determines the overall organization of the cuts within each cutting pass or cut depth. The pattern that you select also enables or disables other groups of settings on this page.
- Use the Area options to further specify how Mastercam defines the area to be cut during each pass. Select each checkbox that is relevant to your part; as you select each checkbox, Mastercam creates a sub-page in the tree with additional options and settings. Review and complete the options on each sub-page.
- The Sorting options define how Mastercam orders the cuts within each cutting pass. For example, you might want to cut in one direction only, or zig-zag within each pass.
- The Stepover options define the spacing between the cuts at each depth.
- The Surface Quality options control how closely the cutting passes fit your part model. Additional options are on the Advanced Options for Surface Quality page.
Type
The pattern type determines the overall organization of the cuts during each cutting pass.
- Offset: The tool follows a contour of the part model at the cutting depth, with each pass offset by the stepover amount.
- Parallel: Each cutting pass is composed of parallel linear cuts.
- Dynamic: Each cutting pass is composed of smooth continuous tool motions, similar to OptiRough or a 2D Dynamic toolpath.
Depth step
The Depth step controls the spacing between each cutting pass or slice as the tool plunges into the part. Choose one of the following options.
- Constant depth step: Specify the distance between each depth step as an absolute value. The depth steps are of equal value throughout the toolpath.
- Number of slices: Specify the number of depth steps or cuts. Mastercam calculates the distance between each step.
Closed offset
Available when the Offset pattern is selected. Select this option to create your cutting passes with closed loops even if you have selected a feature such as an open pocket. Leave this unselected to create open contours or pockets.
Draft angle
Apply a Draft angle to organize the cutting layers so that as you move away from the part, the area enclosed by each pass expands. The result is that the area that is machined above the pocket is conical, rather than cylindrical. One reason to apply a Draft angle is when you will be finishing the part with a tapered tool or with a tool whose axis will be tilted and you want to avoid collisions with the wall material.
Undercuts
Identifies areas with undercuts and includes them in the machined area, and activates the Undercuts page where you can configure which undercut areas will be included in the toolpath. This option is available for the Offset cutting pattern only.
Rest rough
Machine previously uncut areas of the part based on the diameter of the previous roughing tool, and activates the Rest Roughing page where you can configure which areas will be processed.
Containment
Restrict the cutting passes inside a selected curve. This is in addition to the avoidance geometry selected on the Model Geometry page. Activates the Containment page where you can configure how the tool interacts with the containment boundary.
Fixture curves
Lets you select curves or geometry that represent fixtures to be avoided. These function similarly to containment boundaries, except that the tool will stay inside the containment boundary, but outside the fixture curves. Activates the Fixture Curves page where you can configure how the tool interacts with the boundary.
Silhouette containment
Creates a containment boundary based on the silhouette of the surfaces or model that is being machined. Activates the Silhouette Containment page where you can configure how the boundary will be created.
Cutting method
Select the cutting method from the drop-down list. Not all of these options are available for all cutting patterns.
- One way: The tool cuts each pass in the same direction.
- Zigzag: The tool cuts each pass in the opposite direction from the previous one.
- Spiral: The tool cuts in a spiral motion on the part.
Direction for closed cuts
Defines the direction of the tool movement relative to the rotation direction of the spindle.
- Climb: The tool moves in the same direction as the spindle rotation.
- Conventional: The tool moves in the opposite direction of the spindle rotation.
Feed rate (conventional)
Sets an alternate feed rate for the conventional motion of a zigzag cut. If this option is set to zero, Mastercam substitutes it with the standard feed rate. This option is only available when the Cutting method is set to Zigzag.
Machine by
Select an option from the drop-down list. Not all options are available for all cutting patterns.
- Levels: Cuts the part by alternating between pockets for each level.
- Regions: Splits the toolpath into regions when the tool encounters a gap. Use when the part geometry creates excessive air motion around gaps.
Intermediate slices
Processes intermediate slices After each depth step or After last depth step.
- After each depth step: Processes intermediate slices after each corresponding regular slice.
- After last depth step: Processes intermediate slices after the last regular slice is cut.
Start point
Select this option to activate the Start Point page, where you can select the start point. This is not an actual location on the toolpath or part geometry, but an indication to Mastercam of where you would like the toolpath to begin (for example, the right or left side of the part, or near a specific feature). This is often a point in space near the place where you would like to begin cutting.
Reverse order
Reverses the toolpath sorting.
Cut tolerance
Determines the accuracy of the toolpath. A smaller cut tolerance creates a more accurate toolpath, but may take longer to generate the toolpath and will create a longer NC program.
Damp
Smooths abrupt transitions in the tool angle by inserting fillets in the toolpath. The radius of the fillets is twice the diameter of the tool.
The Stepover fields are linked, so that when you make a change in one field, Mastercam updates all the fields. This lets you specify the stepover distance in whichever way makes the most sense for your application.
Maximum stepover
Enter a value for the maximum distance between passes at the cut depth.
Scallop height
Specifies the height of the remaining material between passes when using a rounded tool. Mastercam calculates the stepover based on the value that you enter here and the diameter of the selected tool.
Tool diameter %
Specifies the stepover as a percentage of the diameter of the selected tool.





