Cut Pattern: Pocketing
Use this page to establish the cut pattern parameters for your Multiaxis Pocketing toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.
Common Toolpath Parameter Controls
Machining geometries
Click the Select arrow button to return to the graphics window for surface selection.
Click the Clear all arrow button to deselect all previous selections.
Floor geometries
Click the Select arrow button to return to the graphics window for surface selection.
Click the Clear all arrow button to deselect all previous selections.
Wall geometries
Click the Select arrow button to return to the graphics window for surface selection. The Wall geometries option appears only when Machining is set to Floor finishing or Wall finishing.
Click the Clear all arrow button to deselect all previous selections.
Ceiling geometries
Click the Select arrow button to return to the graphics window for surface selection. Ceiling geometries only appears when Machining is set to Roughing and Strategy is set to Offset from ceiling or Morph between ceiling and floor.
Click the Clear all arrow button to deselect all previous selections.
Stock to leave
Enter the amount of material to leave on the part model when the operation is finished.
Machining
Choose the type of machining (Roughing, Floor finishing, or Wall finishing) you want to do with this toolpath.
Strategy
Choose a machining strategy from the drop-down list.
- Offset from floor: All cuts are parallel to the floor.
- Offset from ceiling: All cuts are parallel to the ceiling.
- Morph between ceiling and floor: Cuts are a blend between the floor and ceiling.
- Parallel: Each cutting pass is composed of cuts parallel to the selected guide curve.
Guide curve
Specifies the type of guide curve used when you set Strategy to Parallel. The choices are as follows:
- Longest dimension: The longest dimension from the floor surface.
- User defined curve: Allows the user to define one or more drive curves. Clicking the selection arrow returns you to the graphics window to select the curves.
Type
Select the method for cutting the toolpath area from the drop-down list. Determines where the tool starts, ends, and the area that is machined.
Cutting method
Select the cutting method from the drop-down list. Depending on the Machining setting, choose between the following:
- 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 feeds into the part in a continuous spiral.
Feed rate (conventional)
Use this option to set 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. Only available when Cutting method is set to Zigzag.
Direction for one way machining
Select Climb or Conventional from the drop-down list to set the cutting direction.
Machine by
Select an option from the drop-down list.
- 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.
Rest rough
Select to activate the Rest Roughing page of the tree structure. Use to machine previously uncut areas of the part based on the previous roughing tool diameter.
Containment
Select to activate containment. Click Select to select a chain to control the cutting area of the part.
Undercuts
Specifies the setting for undercuts, the choices being No , Yes , and Machine Only.
Extend undercuts
When choosing to machine only undercuts, extends the boundary of the undercut to ensure a smoother transition from the non-undercut area. To enable this parameter, set Type to Offset and Undercuts to Machine only.
Avoid undercuts
Specifies an additional avoidance distance to avoid undercuts.
Constant depth step
Enter the distance between depth steps. The depth steps are of equal value throughout the toolpath.
Number of slices
Enter a maximum amount of depth cuts to the toolpath.
No. of intermediate slices
Enter the number of slices to create between depth steps. Use to reduce the size of cusps created on angled surfaces when pocketing.
Cut tolerance
Enter a tolerance value to set the surface quality.
Maximum stepover
Enter a value for the maximum distance between cutting passes.
Desired stepover
Enter the targeted stepover for the toolpath motion. The stepover value is adjusted up to the maximum stepover while trying to maintain the desired stepover.
Climb stepover (% stepover)
Enter a percentage of the stepover to use when climb motion is used in the toolpath.
Conventional stepover (% stepover)
Enter a percentage of the stepover to use when conventional motion is used in the toolpath.





