G-Code Reference for CNC Machines

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.

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).

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+).

Was this article helpful?