The field to the right of Cutter Compensation is the Side Clearance Amount and is active with all following options that contain Clearance or Compensation.
Offset - SURFCAM offsets the toolpath by the tool radius. Gouge avoidance is controlled in SURFCAM.
Offset with Clearance - SURFCAM offsets the toolpath by the tool radius, and applies a side clearance move at the entry and exit locations, perpendicular to the toolpath. The length of the side clearance move equals the Side Clearance Amount plus the Finish Spacing (On Side). Gouge avoidance is controlled in SURFCAM.
Offset with Compensation - SURFCAM offsets the toolpath by the tool radius, and applies a side clearance move at the entry and exit locations, perpendicular to the toolpath. The length of the side clearance move equals the Side Clearance Amount plus the Finish Spacing (On Side). The output NC code includes a Comp Left or Comp Right command (typically G41, G42) at the beginning of the entry side clearance move, as well as a Comp Off command (typically G40) at the end of the exit side clearance move.
Part/Edge (Contour only) - SURFCAM drives the tool directly along the part geometry, in the direction defined by Cutting Method (Climb or Conventional) and on the offset side chosen. Gouge avoidance is inactive.
Part/Edge with Clearance (Contour only) - This works the same as the Part/Edge option, but with side clearance move equal to the Side Clearance Amount applied at the entry and exit locations. The side clearance move is perpendicular to the toolpath in the offset direction.
Part/Edge with Compensation (Contour only) - SURFCAM drives the tool directly along the part geometry, in the direction defined by Cutting Method (Climb or Conventional) and on the offset side chosen. Gouge avoidance is inactive. A side clearance move equal to the Side Clearance Amount plus the tool radius is applied at the entry and exit locations, perpendicular to the toolpath in the offset direction.
The NC code includes a Comp Left or Comp Right command (typically G41, G42) at the beginning of the entry side clearance move, as well as a Comp Off command (typically G40) at the end of the exit side clearance move.
If you use an Arc Leadin with Part/Edge programming, the actual radius at the NC machine after cutter compensation equals the Leadin Radius minus the cutter radius. This way, the specified radius appears in the GCode, even though the machine move after cutter compensation will not reflect this value.