Cut Pattern: Port
Use the Cut Pattern page to establish the cut pattern parameters for your Multiaxis Port toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.
Common Toolpath Parameter Controls
Surfaces
Returns you to the graphics window for surface selection. Multiple surfaces may be selected provided the surfaces form a contiguous row, or where the surface directions are not in conflict with one another. The number of surfaces selected is displayed to the left of the button.
Flow parameters
Opens the Flowline data dialog box if a surface has already been selected. Use the buttons to toggle offset, cut direction, step direction, and start position. Enter a value for your edge tolerance. You may also use the Plot edges button to see the surface edges plotted in various colors.
Cutting method
Use the drop-down selection to choose Zigzag, One way, or Spiral. The selection generates tool motion as described by the name.
Compensation type
Choose how you want to handle Compensation type:
- Computer: Mastercam computes the compensated toolpath and does not output control codes for compensation.
- Control: Mastercam outputs control codes for compensation and does not compute the compensated toolpath.
- Wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are the same.
- Reverse wear: Mastercam both computes the compensated toolpath and outputs control codes for compensation. Compensation direction in the computer and control are opposite.
- Off: Mastercam programs the tool tip directly on the chained geometry and does not output compensation codes. The options that are available to you are determined by the active control definition.
Compensation direction
Offsets the tool to the right or left of the toolpath. Even if Compensation type is set to Off, Mastercam uses this setting to determine the orientation of other toolpath features such as multiple passes.
Tip compensation
Sets amount of offset to the tool's center or tip for bull-nose and ball (spherical) tools. Used for touching the tool off the part. Outputs the tool tip offset as either the tip or the corner radius distance from the tip.
Stock to leave on drive surfaces
Specifies how much stock to leave on the drive surfaces for a subsequent finish operation. This is a 3D distance measured normal to the surface.
Diameter (for simulation)
Only available when Compensation type is set to Control, Wear, or Reverse wear. Enter a value to be used by Classic Backplot and Mastercam Simulator to represent a control compensated tool. The field is initially given the value of the tool selected for the operation, with the ability for the user to override this value.
Distance increment
Enable the checkbox and enter a distance value. The value is a linear distance along the path taken by the tool. An additional vector will be added to the toolpath when the distance between calculated vectors is greater than the distance increment value.
Distance (Step along)
Use a distance value to limit tool motion. The specified value is the distance between generated vectors along the selected geometry. A smaller value creates a more accurate toolpath, but may take longer to generate and may create a longer NC program.
Cut tolerance
Determines the accuracy of the toolpath. A smaller cut tolerance value creates a more accurate toolpath, but may take longer to generate the toolpath and create a longer NC program. This value is also used to eliminate duplicate positions and as a tolerance when compensating to surfaces.
When Distance is deselected, Mastercam uses the cut tolerance you specify as a tolerance to fit tool positions to the surface based on the curvature of the surface. Otherwise, Mastercam uses the Distance value as an absolute distance for the space between each tool position.
Distance (Step across)
Enter a value to control the distance between passes. Use Distance when you need to have control of the stepover amount.
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.





