G40, G41, G42: cutter radius compensation

A program describes the part, but the centre of a milling cutter has to run one radius away from it. Cutter radius compensation lets the control do that offset: the program follows the contour, and the tool’s radius sits in the control’s offset table. On a Haas, in Productivity’s training manual (2026 edition; quotes below are from it unless marked 2025), “A G41 or G42 command must include a Dnnn value to select the correct offset from the tool offset table.” What D means differs by control: on LinuxCNC it is an optional tool number (“If supplied, the D word is the tool number to use.”), on Siemens the tool offset that also switches on length compensation. LinuxCNC’s advice for the first line: “Start a program with G40 to make sure compensation is off.” For the motion codes the compensation acts on, see G00, G01, G02, G03.

Left or right

The side is seen from behind the tool, looking the way it moves. LinuxCNC: “G41 is your left side of the line and G42 is the right side of the line.”; Siemens: “G41 Call for cutter path compensation, tool in traversing direction left of contour”. LinuxCNC and Yaskawa define G40 as switching it off. Reverse the direction of travel and the same side of the part becomes the other code, so an outside contour run one way needs G41 and run the other way G42.

Productivity’s 2026 Haas manual labels the two “G41 (Climb Milling)” and “G42 (Conventional Milling)”; its 2025 edition defines them by direction only. A Mastercam trainer says the same: “typically CNC use a climb cut which is offset left, or G41” (camInstructor). The pairing holds for a spindle turning clockwise (M03) with a right-hand cutter: on the left of the contour, its teeth at the cut move the same way as the work moves relative to the tool. That condition is this page’s reasoning; no source read for this page states it. The difference between the two is on the climb vs conventional milling page.

G41 · leftG42 · right, reversedG42 · right, same direction

Program (FANUC/Haas style)

1. N10 G00 X14. Y110.
2. N20 G41 D01 G01 X45. Y60. F500
3. N30 X150.
4. N40 G03 X170. Y80. R20.
5. N50 G01 Y140.
6. N60 X270.
7. N70 G40 G01 X302. Y182.

Outside cornerarc (G450)intersection (G451)

Tool radius

8

mm

Turning it on and off

• On a straight move. Productivity: “Cutter compensation cannot be turned ON or OFF during a G02 or G03 arc move.”; LinuxCNC lists “A G2/G3 arc move is programmed next after a G40.” among its errors. Productivity’s lathe manual allows the approach as “a linear move, that is a G01 or G00”; its mill manual asks for “a G01 X,Y move”.
• At least one radius long. LinuxCNC: “The lead in move must be at least as long as the tool radius.”; Productivity: a move “equal to or greater than the cutter radius”, and, in a thread-milling note, that it works “as long as the move is greater than the amount being compensated”. LinuxCNC adds that the lead-in should suit “the largest tool radius that might be used”.
• Out the way it came in. Productivity: “The entry and exit moves must follow the same rules—what is put in must be taken out.” LinuxCNC is stricter on the way out: “If tool compensation was on the next move must be a linear move and longer than the tool diameter.”
• Approach on Siemens. “NORM The tool travels directly along a straight line and is perpendicular to the contour point.”; “KONT The tool travels around the contour point in accordance with the programmed behavior at corners G450/G451.”
• Not left on. A program stopped with compensation active gives the alarm “349 PROG STOP W/O CANCEL CUTTER COMP” on a Haas (Haas workbook; Productivity), and “Pressing RESET or POWER OFF will also cancel cutter compensation.” (Haas). These numbers are from older Haas lathe documents.

Corners and small arcs

On an outside corner the offset lines leave a gap, and controls close it in one of two ways. Siemens: “G450 Transition circle, the tool travels around workpiece corners along a circular path with tool radius.” and “G451 Intersection point, the tool cuts free in the workpiece corner.” On a Haas, Setting 58 chooses: in YASNAC mode “A circular motion joins all of the outside angles.”; in Fanuc mode “The control joins outside angles less than or equal to 270 degrees with a sharp corner”, and larger ones with “an extra linear motion” (Productivity, 2025 edition). Yaskawa’s control can likewise insert a blending arc or extend the lines to their intersection.

On an inside corner the offset lines overlap, and the control has to trim them, or stop. LinuxCNC: “If the next move creates in an inside corner the move will stop short so to not gouge the part.” Haas, in Productivity’s manual: “if the programmed path would cause an overcut, the control will stop and issue an alarm”, and “machining an inside arc with a radius smaller than the active D-value will generate an alarm”. Siemens has collision detection switched with CDON and CDOF: “The control detects and corrects critical machining situations.”

To see these situations coming, the control reads ahead. Productivity’s 2026 manual: the Haas control “looks ahead to the next two blocks containing X or Y motion to check for interference”. How other controls count, and what blocks without motion in between do, was not found in the sources read for this page.

Geometry, wear, diameter or radius

On a Haas, “Total compensation is the sum of the geometry and wear values.”, and “The offset may be specified as either a Diameter or a Radius, depending on Setting 40.”; with diameter, “the shift amount is half of the value entered” (Productivity, 2025 edition). LinuxCNC keeps a diameter in its tool table, “a positive real number representing the measured diameter of the tool”, and G41.1/G42.1 take the diameter in the block itself. On Siemens, “The tool length compensation acts automatically after tool offset D has been called.”

CAM systems offer the same choice in five settings. Fusion’s names are first, Mastercam’s (as a trainer describes them) second:

Fusion applies the control settings only on finishing passes (Fusion help).

Planes

Compensation works in one plane at a time. Productivity: “Cutter compensation is available in X and Y for 2D machining (G17), and in X, Y, and Z for 3D machining with G141.” LinuxCNC: “Cutter compensation may be performed if the XY-plane or XZ-plane is active.”; with YZ it gives an error.

On the lathe: tool nose radius compensation

A turning insert has a nose radius, but the offsets measure an imaginary point: the geometry offsets “intersect at a point, called the IMAGINARY TOOL TIP” (Productivity). Along X or Z alone it generally does not need to be used (Productivity); “For taper and circular cuts, as the tool nose radius changes, under or overcutting can occur.” (Productivity). The same codes do the correction: “G41 Tool Nose Compensation LEFT of the programmed path”, “G42 Tool Nose Compensation RIGHT of the programmed path” (Haas), and “normal I.D. turning will require a G41”, normal outside turning from the face toward the chuck G42 (Productivity). The control also needs the direction of the nose, “coded as a single integer from 0 to 9”, where “Zero (0) indicates no Specified direction.” (Productivity).

The approach and departure moves “should be equal to or greater than the tool nose radius of the tool”, with twice that on X moves because X is programmed as a diameter; too short a move gives “alarm (369 TOOL TOO BIG)” (Productivity). Productivity’s lathe manual also has compensation cancelled before the canned cycles G74, G75, G76 and G92, which ignore it.