Use this page to
establish the cut pattern parameters for your Multiaxis Multisurface toolpath. Cut pattern settings
determine the geometry your tool follows and how it travels along
that geometry.
Common Toolpath Parameter Controls
Pattern options
Controls the tool motion according to the selected shape. The chosen option dictates the behavior of the Select button as follows:
- Surfaces: Click Select to return to the graphics window for surface selection. The number of surfaces selected is displayed to the right of the Select button.
- Cylinder / Sphere / Box: Click Select to open a corresponding dialog box. Use the dialog box to enter parameters for the selected shape.
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
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.
Distance increment
Select the checkbox and enter a 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.
Cut tolerance
Determines the accuracy of the multiaxis 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.
Across stepover
Enter a value to control the distance between passes. A smaller value creates more passes, but may take longer to generate and may create a longer NC program.
Along stepover
Enter a value used to limit tool motion. The value specified 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.
Flow parameters
Opens the Flowline data dialog box. 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.
Diameter (for simulation)
Only available when Compensation type is set to Control, Wear, or Reverse wear. Enter a value to be used by Backplot and Verify 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.