Pattern Repeat Parameters
Use the options on this tab to create a pattern repeat toolpath for roughing applications. Each cutting pass will offset the part contour according to the dimensions that you enter here.
This toolpath typically produces canned cycle output if your control supports it. You can select Permanently change to longhand to change the NC output to individual position moves instead of the canned cycles.
Pattern offset angle
Enter the angle at which the cutting passes will be offset from the original contour. This angle is typically measured relative to the Z or spindle axis.
Permanently change to longhand
Select to disable the canned cycle output. Instead of outputting a single canned cycle G-code with its parameters, your NC program will contain all of the individual position moves.
Once you generate the toolpath with this option selected, you will not be able to change back to canned cycle output.
Stepover
Enter the amount of stock to remove from the diameter with each pass.
Number of passes
Enter the number of passes to create. Mastercam multiplies this number by the Stepover and then adds the Stock to leave, to calculate how much total stock it needs to remove in this operation.
Stock to leave in X
Determines how much stock remains in the X direction when the operation is finished. Typically, this would be removed by a separate finish operation.
Stock to leave in Z
Determines how much stock remains in the Z direction when the operation is finished. Typically, this would be removed by a separate finish operation.
Compensation type
Tool compensation adjusts the toolpath to allow for the cutting tool's radius. The options that are available to you are determined by the active control definition.
- 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.
Optimize cutter compensation in control
Eliminates arcs in the toolpath that are less than or equal to the radius of the tool and helps prevent gouging. The default setting for this field is set on the Cutter Compensation, General page in the Control Definition. This field is available only when Cutter compensation is set to Control on the parameters tab, and applies only to that setting.
Roll cutter around corners
Inserts arc moves around the corners in the toolpath. Choose the type of arc move:
- None: Guarantees all sharp corners.
- Sharp: Only rolls the tool around sharp corners of 135 degrees or less.
- All: Rolls the tool around all corners and creates smooth tool movement. The radius of the arc moves equals the radius of the tool.
Lead In/Out
Select to add lead in or lead out moves to the toolpath and click to edit the moves.
Extend contour to stock
Extends the contour established by the part geometry to the stock boundary. Click Adjust Contour Ends to control how the contour is extended. This option is available only if stock for the current active spindle is defined in Machine Group Properties and the chained contour lies entirely within the stock boundary.
Adjust contour ends
Opens the Adjust Stock dialog box where you adjust the area of the stock to be removed by extending the chained contour to the stock boundary. This option is available only if stock for the current active spindle is defined in the machine group properties and the chained contour lies entirely within the stock boundary, and if Extend Contour to Stock is checked.
Linearization tolerance (Only available when chaining splines)
Used when converting 3D arcs and 2D or 3D splines in the chained geometry from curves to lines. Smaller linearization tolerance values make more accurate toolpaths, but may take longer to generate and create a longer NC program.





