Finish Parameters: PrimeTurning™
Use the options on this tab to create a finish PrimeTurning toolpath for your part. Enter your cutting parameters in the fields, and choose an orientation for the toolpath in the Cut direction drop-down list. You can also enable the additional options and advanced features on the right side of the tab.
Finish
Activates the finishing page of options.
Finish stepover
Select to create one or more finish passes. Enter a stepover distance to define how much stock gets removed during each finish cut.
Number of finish passes
Enter the number of finish passes. If you choose to make more than one finish pass, Mastercam determines the offset direction automatically.
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.
Feed rate
Specifies the feed rate for the finishing passes. You can choose measurements per revolutions or minutes, or a finish in Microns.
Spindle speed
Determines the rotation speed of the spindle in revolutions per minute (RPM) or constant surface speed (CSS). Mastercam calculates a default value according to the machine group properties, but you can override this by typing in a new value. If you are in RPM mode, Mastercam warns you if either the default or the value you type in is outside the range set in the machine definition.
Cut direction
Choose from which direction the tool cuts the toolpath: ID, OD, face, or back.
Compensation type
The options that are available here are determined by the active control definition. Choose one of the following:
- 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
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 General page in the Control Definition dialog box.
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.
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.
Down cutting
Select to activate down cutting. Select the button to open the Down Cutting Parameters dialog box.
Corner break
Select to automatically create radii or chamfers on all outer corners of the toolpath. Select the button to open the Corner Break dialog box.
Lead in/out
Select to have Mastercam add lead in/out moves to the toolpath. Select the button to open the Lead In/Out dialog box.
Plunge parameters
Opens the Plunge Cut Parameters dialog box, which defines how the tool handles undercuts on the toolpath along each axis.
Filter
Select to eliminate unnecessary tool moves in the toolpath to create smoother movement. Select the button to open the Filter dialog box.
Tool inspection
Select to turn on tool inspection. Select the button to open the Tool Inspection dialog box.
Chip break
Select to identify when chip breaks can occur. Select the button to open the Chip Break dialog box.
Stock recognition
Stock recognition is locked to Remaining stock in the PrimeTurning toolpath. The Remaining stock setting uses only stock remaining from previous operations.
Adjust stock
Opens the Adjust Stock dialog box and lets you adjust the area of the stock to be removed by the finish operation. This option is available only if:
- You define stock boundaries in the machine group properties.
- The chained contour lies entirely within the stock boundary.
- You select either the Use Stock for Outer Boundary or Extend Contour to Stock Only options.





