Cut Pattern: Port Expert
Use the Cut Pattern page to establish the cut pattern parameters for your Multiaxis Port Expert toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.

Common Toolpath Parameter Controls
Pattern
Select a pattern from the drop-down list. Two additional options are available if you choose Roughing:
- Offset creates traditional roughing passes offset from the part or model.
- Dynamic creates more aggressive roughing passes similar to Mastercam's other Dynamic Roughing toolpaths.
Machining surfaces
Click the Select arrow button to close the dialog box, and then select surfaces from the graphics window. When you have completed selection in the graphics window, press End Selection to return to the dialog box.
Click the Clear all arrow button to deselect all previous selections.
Offset
Specifies the amount of rest material to leave when machining.
Automatic spine
Allows Mastercam to calculate the spine for the toolpath. When deselected, Click the Select arrow button to close the dialog box, and select the spine geometry. When you have completed selection in the graphics window, click OK to return to the dialog box.
Click the Clear all arrow button to deselect all previous selections.
Output type
Use the drop-down list to select Both, Top, or Bottom. Mastercam calculates the entire port toolpath but you have the ability to output either half or the complete toolpath.
Machine to
Select an option from the drop-down list. The selection is used as the endpoint of the toolpath within the port.
Top
Adjust the slider to specify the portion of the top port area to be machined. Zero percent represents the top of the port area, and 100 percent represents the midpoint of the port area.
Bottom
Adjust the slider to specify the portion of the bottom port area to be machined. Zero percent represents the midpoint of the port area, and 100 percent represents the bottom of the port area.
Cutting method
Select the cutting method from the drop-down list.
- 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.
Direction for one way machining
Set the cutting direction to Climb or Conventional from the drop-down list.
Ramp angle
Enter the angle of the entry helix to be used as the tool enters the port.
Cut tolerance
Determines the accuracy of the toolpath. A smaller cut tolerance value creates a more accurate toolpath, but may take longer to generate and create a longer NC program.
Maximum distance
Enable the checkbox and enter a value for the maximum distance between toolpath positions in the cutting direction. Use in operations where you need to have more points defined, such as on flat surfaces.
Minimum distance
Enable the checkbox and enter a value for the minimum distance between toolpath positions in the cutting direction. Use in operations where you need to have more points defined, such as on flat surfaces.
Damp
Allows a more flexible application of the axial shift.
Maximum stepover
Enter a value for the maximum distance between cutting passes.
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 selected tool. The Maximum stepover and Scallop height fields are linked so that when you type a value in one field, Mastercam automatically updates the other.
Depth step
Enter the distance between roughing passes.





