Cut Pattern: Rotary
Use this page to establish the cut pattern parameters for your Multiaxis Rotary toolpath. Cut pattern settings determine the geometry your tool follows and how it travels along that geometry.
Common Toolpath Parameter Controls
Surface
Click Select to return to the graphics window for surface selection. The number of surfaces selected is displayed to the right of the button.
Cutting method
Click the radio button to select the desired cutting motion.
- Rotary cut: The tool travels around the circumference of the part. After each pass around the part, the tool moves along the axis of rotation for a subsequent pass.
- Axial cut: The tool travels parallel to the axis of rotation. After each pass parallel to the axis, the tool moves around the circumference for a subsequent pass.
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
Choose to offset 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
Use this option to specify how much stock to leave on the drive surfaces for a later finish operation. This is a 3D distance measured normal to the surface.
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 create a longer NC program. This value is also used to eliminate duplicate positions and as a tolerance when compensating to surfaces.
When the Distance checkbox 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.
Reverse cut direction
Flips the direction of the toolpath from the default. The toolpath cuts in the opposite direction, starting from the opposite end of the geometry.
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.
Direction of closed contours
Click the radio button to select the desired cutting motion for closed contours, which form a continuous loop.
- Climb: The tool engages the material so that the maximum chip thickness is at the beginning of the cut. The chip thins as the tooth approaches the work piece, resulting in a smoother finish. Tool life may be extended at the expense of machine load.
- Conventional: The tool engages the material so that the maximum chip thickness is at the end of the cut. The chip thickens as the tooth moves away from the work piece, which can result in a rougher finish. The initial chip thinness may result in dulling of the tool, as well as work-hardening the material.
Direction of open contours
Click the radio button to select the desired cutting motion for open contours, which have distinct start and end locations.
- One way: The tool engages the material in a single direction. The tool is not in contact with the material as it returns to the next start location.
- Zigzag: The tool engages the material in both directions. The tool is in contact with the material as it returns in the opposite direction.





