Finish Pencil Parameters
Use this tab to define the machining direction, bitangency angle, and, optionally, the number of parallel passes for a Finish Pencil toolpath. Pencil toolpaths travel along the interior edges between surfaces.
Total tolerance
Displays the sum of the Cut tolerance, the Line/arc tolerance, and Smoothing tolerance. Click Total tolerance to open the Arc Filter/Tolerance dialog box. Use the options in this dialog box to set parameters for filtering and smoothing toolpath motion within the specified total toolpath tolerance.
Parallel passes
Allows you to choose whether to create parallel passes. A parallel pass is a cutter path that you offset from the central pencil trace by a given amount (the stepover). A pencil trace is the path along which the cutter maintains contact with the drive geometry in at least two distinct points. Choose one of the following options.
- None: Creates a single pencil toolpath, disabling parallel passes.
- Number per side: Allows you to enter the number of parallel passes to crate on each side of the central pencil trace, offset by the value you enter in the Stepover field.
- Unlimited: Creates parallel passes all the way across the selected drive geometry offset by the value you enter in the Stepover field.
Use approximate start point
Allow negative Z motion along surface
Lets the tool cut along the surface while plunging. Deselect this option if you are using a tool that does not cut downward.
Allow positive Z motion along surface
Lets the tool cut along the surface while retracting. Deselect this option if you are using a tool that does not cut upward.
Bitangency angle
Specifies how shallow the corner or angle between two surfaces needs to be in order for Mastercam to create a cutting pass. Use this to prevent cutting passes where the transition between two surfaces is flat or nearly flat. A typical recommended value is 165 degrees.
Overthickness
Use this option to increase the apparent size of the cutter to force a cutting pass when one would not ordinarily be created. This can also be useful when the size of the cutter is equal to, or very close to, the size of the fillet; entering an Overthickness amount greater than the Cut tolerance helps ensure that Mastercam will create a smooth continuous pass through the pencil zone.
Cutting method
Orients the cutting direction. Select one of the following options:
- Zigzag: Cuts each pass in the opposite direction to the previous pass. A short linking motion connects the two ends.
- One Way: Cuts one direction, steps over to the next cut while making a rapid move to same start side of the cut, and cuts in the same direction as the previous pass.
Machining direction
Sets the machining direction of the toolpath. Select one of the following:
- Climb: Cuts in one direction with the tool rotating in the opposite direction of the tool motion.
- Conventional: Cuts in one direction with the tool rotating in the same direction as the tool motion.
Deselecting Machining direction allows both Climb and Conventional cuts in the toolpath. In some cases, this allows the tool to cut more of the part than possible when the tool must move only in a climb or conventional manner. Useful when the tool is not allowed to cut up or down along the part.
Depth limits
Sets the minimum and maximum machining depths for the toolpath. Click Depth limits to open the Depth limits dialog box.
Gap settings
Sets the handling of motion when there is a break in the tool motion, such as between two surfaces. Click Gap settings to open the Gap Settings dialog box.
Advanced settings
Sets tool roll motion at sharp corners between surfaces and at the extreme edges of the part, the corner tolerance, and performs checks on solid and surface models. Click Advanced settings to open the Advanced settings dialog box.





