G-Code Reference for CNC Machines
G-code and M-code command reference for CNC milling, turning, and 3D printing machines. Includes motion, work offsets, spindle, coolant, and common program structure.
Reference
G-code (ISO 6983 / RS-274) is the canonical language for CNC controllers. Commands are grouped into modal groups — once set, a G-command stays active until another command in the same group replaces it. Exact dialects vary between controllers (Fanuc, Haas, Mazak, LinuxCNC, GRBL, Marlin); this page covers the common core.
Motion (G-codes, modal group 1)
| Code | Name | What it does |
|---|---|---|
| G00 | Rapid move | Traverse at max machine feed, no cutting. Non-linear path on most controllers. |
| G01 | Linear feed | Straight line at programmed feedrate (F). Used for cutting. |
| G02 | CW arc | Clockwise circular interpolation. Needs I/J/K (center offset) or R (radius). |
| G03 | CCW arc | Counter-clockwise circular interpolation. Same params as G02. |
| G04 | Dwell | Pause for P seconds or X seconds. Used after spindle commands. |
| G05.1 | Look-ahead | Fanuc AI contour / high-speed. Q1 on, Q0 off. |
| G33 | Thread cutting | Lathes — synchronised feed to spindle. K = thread pitch. |
| G73 | Peck drill (high speed) | Partial retract cycle. Fast chip clearing. |
| G76 | Fine bore | Boring cycle with oriented spindle stop and shift. |
| G80 | Cancel canned cycle | Ends drill/tap/bore cycles (G81–G89). |
| G81 | Drill canned cycle | Simple drill-to-Z-then-retract. |
| G82 | Drill + dwell | Counterbore: drill, dwell P, retract. |
| G83 | Peck drill | Retract-to-R-plane between pecks for deep holes. |
| G84 | Tapping cycle | Synchronised tap. Requires rigid-tap-capable spindle. |
| G85 | Boring | Feed in, feed out (no dwell). |
Plane / units / mode (modal groups 2, 6, 3)
| Code | Group | Meaning |
|---|---|---|
| G17 | Plane | XY plane (mill default). Arcs use I/J. |
| G18 | Plane | XZ plane (lathe default). Arcs use I/K. |
| G19 | Plane | YZ plane. Arcs use J/K. |
| G20 | Units | Inches. |
| G21 | Units | Millimetres. |
| G90 | Distance | Absolute positioning (X = absolute coord). |
| G91 | Distance | Incremental positioning (X = distance from current). |
| G93 | Feed mode | Inverse time — F = 1 / minutes per move. |
| G94 | Feed mode | Feed per minute (in/min or mm/min). Default on mills. |
| G95 | Feed mode | Feed per revolution. Standard on lathes. |
Tool & cutter compensation (groups 7, 8)
| Code | What it does |
|---|---|
| G40 | Cancel cutter-radius comp. |
| G41 | Cutter comp left of programmed path (climb milling, RH tool). |
| G42 | Cutter comp right of programmed path (conventional milling, RH tool). |
| G43 | Tool-length comp positive (H word gives offset number). |
| G44 | Tool-length comp negative (rare). |
| G49 | Cancel tool-length comp. |
Work coordinate systems (group 14)
| Code | Meaning |
|---|---|
| G53 | Machine-zero coordinates (absolute, non-modal). |
| G54 | Work offset 1 (default on power-up for most controllers). |
| G55 | Work offset 2. |
| G56 | Work offset 3. |
| G57 | Work offset 4. |
| G58 | Work offset 5. |
| G59 | Work offset 6. |
| G54.1 P1..P48 | Extended work offsets (Fanuc). |
M-codes (miscellaneous / machine functions)
| Code | What it does |
|---|---|
| M00 | Program stop (wait for operator). |
| M01 | Optional stop (runs only if "optional stop" is on). |
| M02 | End of program (no rewind). |
| M03 | Spindle on, clockwise. Usually with S (rpm). |
| M04 | Spindle on, counter-clockwise. |
| M05 | Spindle stop. |
| M06 | Tool change (typically preceded by T#). |
| M07 | Mist coolant on. |
| M08 | Flood coolant on. |
| M09 | Coolant off. |
| M19 | Spindle orient (for boring/indexing). |
| M30 | End of program + rewind. |
| M41/M42 | Low/high spindle gear (lathes). |
| M48/M49 | Feed/speed override enable / disable. |
| M98/M99 | Call sub-program / return. |
Address letters (parameters)
| Letter | Typical use |
|---|---|
| X Y Z | Linear axes. |
| A B C | Rotary axes around X, Y, Z. |
| U V W | Secondary linear axes (also incremental in some dialects). |
| I J K | Arc centre offset from start point (IJ for G17, IK for G18, JK for G19). |
| R | Arc radius, also retract plane in canned cycles. |
| F | Feedrate (in/min or mm/min; per rev with G95). |
| S | Spindle speed (rpm) or surface speed (with CSS mode). |
| T | Tool number (plus M06 to execute change). |
| H / D | Tool length offset number (H) / diameter offset number (D). |
| N | Block/sequence number. |
| P Q | Parameters — dwell time (P in G04), subprogram number, cycle peck. |
| L | Loop / subprogram repeat count. |
Minimal mill program — face a rectangle
% O0001 (FACE 60X40) G21 G17 G40 G49 G80 G94 ; mm, XY, clear comps G90 G54 ; absolute, WCS 1 T1 M06 ; face mill, tool change G43 H1 ; tool length comp S3000 M03 ; spindle on CW 3000 rpm M08 ; flood on G0 X-10 Y0 ; rapid to start Z5 ; safe Z G1 Z-0.5 F200 ; plunge X70 F600 ; cut pass 1 Y20 ; step over X-10 ; pass 2 Y40 X70 ; pass 3 G0 Z50 ; rapid up M09 ; coolant off M05 ; spindle off G28 G91 Z0 ; home Z G90 M30 ; end %
Common dialect differences
- Fanuc: most industrial CNC controllers (Mazak, Haas, Doosan, DMG Mori). Uses %…% program delimiters, O#### program numbers.
- Haas: Fanuc-compatible plus Haas-specific G/M codes (G150 general pocket, M95/96, etc.).
- LinuxCNC / Mach3 / Mach4: hobby/retrofit controllers, close to Fanuc but with quirks (support arc R only for < 180°, etc.).
- GRBL: Arduino-based, subset of RS-274. No tool changer, no fixtures beyond G54, limited canned cycles.
- 3D printers (Marlin, Klipper): use G0/G1 + extruder E axis; G28 homing, G29 bed mesh; M104/M109 hotend, M140/M190 bed, M106/M107 fan.
- Always consult the machine builder's manual for exact behaviour — especially of G05.x look-ahead, canned cycles, and macro variables (#100+).
Last updated: