Cutter compensation offsets the lines and arcs of a toolpath to account for the difference between a tool's actual diameter and the diameter specified. For example, if the specified diameter is 0.500, the actual tool diameter, due to wear, could be 0.496. Cutter compensation allows this difference to be accounted for at the control so that a single NC program can be used as long as the tool is close enough in diameter to the ideal size entered into FeatureCAM.
The direction of the compensation depends on the value of Climb mill. If Climb mill is on, the cutter compensation direction is left, and if it is off, the cutter compensation is right.
If you use cutter compensation you must select Enable Cut Comp in Options > Posting. Turning it on does not turn on cutter compensation for every feature, however, as cutter compensation NC code is output only for those features with the Cutter Comp attribute selected. If the Enable Cut Comp option is deselected in Options > Posting, then cutter compensation is disabled for the entire part regardless of the value of the Cutter Comp attributes on each feature.
If you select Part line program, you get a special kind of cutter compensation known as part line programming.
If you have specified both Multiple roughing tools and Part line prog for the roughing pass, then in most cases bad NC code is generated because the first roughing tool is likely to be bigger than the arcs in the part. We would consider this to be a fact of life and you need to turn off one or the other to produce workable NC code.
If cutter comp is not chosen for the roughing, then no cutter comp is output at all.
Cutter compensation for the roughing pass results in only the passes closest to the wall being compensated. The interior passes are not compensated because there is no need.