G40, G41 and G42: Cutter Radius Compensation

Most CAM programs output the path of the tool centre, already offset by the tool's radius. Cutter radius compensation works the other way round: the program follows the outline of the part, and the control offsets the tool by the radius stored in its offset table.

• G41: the tool stays to the left of the path, looking in the direction of travel.
• G42: the tool stays to the right of the path.
• G40: compensation off. The tool centre follows the path exactly.

The D word picks which offset register holds the radius, for example G41 D1.

Why use it

Compensation lets the operator adjust the size of a part at the machine. If a pocket comes out 0.05 mm too small, they change the value in the offset table and run it again, with no trip back to CAM. It also lets one program work with a resharpened or slightly undersize tool.

Many CAM systems offer wear compensation: the program still follows the tool centre path, and the D register holds only a small correction, normally zero. That keeps the program safe to run even if nobody has entered the tool's radius.

Climb or conventional

With the spindle turning clockwise (M3), the side of the path decides the cutting direction:

Lead-in and lead-out moves

The control can't jump the tool sideways by its radius, so it ramps the offset in on the move where compensation turns on and out on the move where it turns off. Those moves need care:

• Turn compensation on during a straight G0 or G1 move, not an arc. Most controls alarm on G41 with G2 or G3.
• The lead-in should be longer than the tool radius and approach the part from outside the material.
• Cancel with G40 on a straight move away from the part, after the last cut.
• Inside corners and slots must be wider than the tool, or the control will stop with an interference alarm.

Example: outside profile of a 40 × 30 mm part

The program follows the part outline, from the corner at X0 Y0 to X40 Y30, clockwise. With the 6 mm end mill's radius (3 mm) in register D1, the control keeps the tool 3 mm outside every edge and climb mills the profile.

(G41 example: outside profile of a 40 x 30 mm part, climb milling)
(The tool radius is stored in D1, so the program follows the part outline)
G21 G17 G90 G54 G40
T1 M6 (6 mm flat end mill)
G0 X-10 Y-10 Z25 S12000 M3
Z5
G1 Z-3 F300
(Lead-in: turn compensation on during a straight move toward the part)
G41 D1 G1 X0 Y-5 F800
Y30
X40
Y0
X-5
(Lead-out: cancel compensation on a straight move away from the part)
G40 G1 X-10 Y-10
G0 Z5
M5
M30

• G41 D1 G1 X0 Y-5 F800 is the lead-in. Compensation ramps in on this straight move toward the part.
• Y30, X40, Y0 and X-5 trace the part clockwise. The last move runs past the starting corner so the edge is cut cleanly.
• G40 G1 X-10 Y-10 cancels compensation on a move away from the part.

Machine differences

• Fanuc and Haas support G41 and G42 with a D register. Haas can store the D value as a radius or a diameter, depending on a setting.
• LinuxCNC uses the tool table and also has G41.1 and G42.1, which take the tool diameter directly on the line.
• Mach3 supports G41 and G42 with its tool table.
• GRBL does not support cutter compensation at all.

How CutViewer shows G40, G41 and G42

CutViewer keeps track of whether compensation is on, but it doesn't apply the offset. It draws the path exactly as programmed, so with G41 or G42 you see the part outline rather than where the tool centre will go. Programs posted with compensation turned off in CAM show the true tool centre path.