Art Base Surface Machining Parameters
Use this tab to enter values for different cutting parameters and compensation options.
Clearance plane
Sets the height at which the tool moves to and from the part. Select the checkbox to activate the clearance height. If the checkbox is not selected, Mastercam uses the Retract plane as the Clearance plane. Click Clearance to set or change the clearance height. You can select a point on the geometry or enter a specific value.
Use clearance only at the start and end of operation
Select this option to rapidly cut to the Clearance plane only at the start and end of the toolpath.
Retract plane
Sets the height that the tool moves up to before the next tool pass. Select the checkbox to activate the retract plane. Then click Retract plane, and select a point on the geometry, or enter a value. Set the retract height above the feed plane.
Feed plane
Sets the height that the tool rapids to before changing to the plunge rate to enter the part. The tool also moves to this height between operations, if you do not enter both the clearance height and the retract height. Click Feed plane and select a point on the geometry or enter a specific value.
Top of stock
Sets the height of the material in the Z axis. Many other toolpath parameters are measured from this position in incremental mode, such as Clearance plane, Retract plane, and Feed planes. Click Top of stock and select a point on the geometry or enter a value. Incremental values are measured from the chained geometry.
Depth
Determines the final machining depth and the lowest depth that the tool descends into the stock. The default depth is the depth of the first chain selected. Click Depth and select a point on the geometry or enter a value. Incremental values are relative to the chained geometry, not the top of stock.
Absolute
Absolute values are always measured from the origin 0,0,0. If you translate geometry associated with a toolpath, and the toolpath depth is set to an absolute value, the tool cuts to that same absolute depth value no matter where the geometry is located.
Incremental
Incremental values are relative to other parameters or chained geometry. Depth and Top of Stock parameters are relative to the location of the chained geometry. Clearance, Retract, and Feed plane are relative to the Top of stock. Note that this parameter does not output incremental coordinates in the NC program. Use the Control Definition Manager to set NC output options.
Tip compensation
Select whether the compensation point will be the center of the tool or the tip. Compensating to the center of the tool is frequently used with ball cutters where compensation will be applied at the control.
Stock to leave (Drive surface)
Gouge checks the selected drive surfaces. Enter a stock to leave amount to prevent the tool from coming close than that distance to the part.
Stock to leave (Check surface/solid)
Gouge checks the selected surface/solid. Enter a stock to leave amount to prevent the tool from coming close than that distance to the part.
Compensate to
Results in a toolpath where the entire tool remains inside or outside the containment boundary, or where the center of the tool travels to the containment boundary.
Additional offset
Enter an additional amount to the tool radius to offset the tool when using Inside or Outside options.





