← AskMachinist · Guides · Calculator · 🔎 Search
Cutter Compensation Basics (G41/G42)
Guide · Updated October 28, 2026
Cutter compensation lets you program the part outline instead of the tool centerline. The control offsets the path by the value in a D register, so you can hold size by changing one number instead of editing the program.
Measure before you adjust
Wear offsets are only as good as the measurement. Check the mic or caliper against gage blocks first. The free Gage Block Calculator builds the stack.
Step by step
- Program the part line: Write the toolpath on the finished contour, not offset by the cutter radius.
- Pick the side: G41 puts the tool to the left of the path (climb milling with a right-hand cutter); G42 puts it to the right (conventional).
- Call the register: Add a D number, e.g. G41 D12, and store the radius or diameter in it, as your control expects.
- Lead in: Turn comp on during a straight move longer than the cutter radius, off the part, before touching the contour.
- Cut the contour: Avoid inside corners or arcs smaller than the tool radius; the control will alarm or gouge.
- Lead out and cancel: Move off the part, then cancel with G40 on another straight move.
- Adjust wear: Measure the part and change the D value, not the program, to bring it to size.
Worked example
A 2.000 in square boss is cut with a 1/2 in end mill, D = 0.2500 (radius mode). It measures 2.0020 in across, so each side is 0.0010 in too big. Lower D to 0.2490 and recut: the tool moves 0.0010 in closer on every side and the boss measures 2.0000 in. For a pocket the logic flips: a pocket that is 0.0020 in small needs D lowered by 0.0010 too, because a smaller D moves the tool outward toward the wall.
Radius vs diameter registers
Some controls store D as a radius, some as a diameter, and some let you set it with a parameter. Check yours: entering a diameter in a radius control doubles the offset and ruins the part.
Common alarms and gouges
"Interference" alarms usually mean an arc smaller than the tool radius or a lead-in too short. A gouge at the start means comp turned on while cutting. Lead-ins along the contour at an angle are safer than straight-on approaches.
Tips
- Lengths: tool length offset basics.
- Measuring: reading an inch micrometer.
- Datums: work offset basics.
FAQ
What is the difference between G41 and G42?
G41 is tool-left of the path, G42 tool-right; with a right-hand cutter G41 climb mills.
Where do I put the D value?
In the tool offset table, as a radius or diameter depending on the control.
Why do I get an interference alarm?
An inside arc or corner is smaller than the cutter radius, or the lead-in is too short.
How do I fix an oversize boss?
Reduce the D value by half the oversize.
Do I need cutter comp on manual-style CAM paths?
CAM can output a centerline path, but using comp in control lets you adjust wear at the machine.
Related guides and calculators
- Tool Length Offset Basics
- How to Read an Inch Micrometer
- Milling Speeds and Feeds
- Carbide End Mill Basics
- Blueprint Reading Basics for Machinists
- Work Offset Basics (G54–G59)
- How to Use a Tool Presetter
- How to Sharpen an End Mill
- Tool Nose Radius Compensation Basics
- CNC G-Code and M-Code Basics
- All free machinist calculators
Build your stack in seconds
The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.
Questions? Ask a machinist.
General shop information only — follow your machine and tooling manufacturer's instructions and your shop's safety rules.