G-Code Quick Reference

G-Codes (Preparatory)

Code	Description	Example
G00	Rapid positioning	`G00 X1.0 Y2.0 Z0.5`
G01	Linear interpolation (feed)	`G01 X2.0 Y3.0 F10.0`
G02	Circular interpolation CW	`G02 X1.0 Y0 I0.5 J0 F8.0`
G03	Circular interpolation CCW	`G03 X1.0 Y0 I0.5 J0 F8.0`
G04	Dwell	`G04 P500` (500 ms)
G10	Data setting (offsets)	`G10 L2 P1 X0 Y0 Z0`
G17	XY plane selection	`G17`
G18	XZ plane selection	`G18`
G19	YZ plane selection	`G19`
G20	Inch mode	`G20`
G21	Metric mode	`G21`
G28	Return to home position	`G28 G91 Z0`
G40	Cutter compensation cancel	`G40`
G41	Cutter compensation left	`G41 D1 X1.0 F10.0`
G42	Cutter compensation right	`G42 D1 X1.0 F10.0`
G43	Tool length compensation +	`G43 H1 Z1.0`
G44	Tool length compensation −	`G44 H2 Z1.0`
G49	Tool length compensation cancel	`G49`
G53	Machine coordinate system	`G53 G00 Z0`
G54	Work coordinate system 1	`G54`
G55	Work coordinate system 2	`G55`
G56	Work coordinate system 3	`G56`
G57	Work coordinate system 4	`G57`
G58	Work coordinate system 5	`G58`
G59	Work coordinate system 6	`G59`
G80	Cancel canned cycle	`G80`
G81	Drill cycle	`G81 X1.0 Y1.0 Z-0.5 R0.1 F5.0`
G82	Spot drill / counterbore (dwell)	`G82 X1.0 Y1.0 Z-0.25 R0.1 P200 F4.0`
G83	Peck drill cycle	`G83 X1.0 Y1.0 Z-1.0 R0.1 Q0.15 F5.0`
G84	Tapping cycle	`G84 X1.0 Y1.0 Z-0.75 R0.1 F25.0`
G85	Bore cycle (feed out)	`G85 X1.0 Y1.0 Z-0.5 R0.1 F4.0`
G86	Bore cycle (rapid out)	`G86 X1.0 Y1.0 Z-0.5 R0.1 F4.0`
G90	Absolute positioning	`G90`
G91	Incremental positioning	`G91`
G92	Set work coordinate offset	`G92 X0 Y0 Z0`
G94	Feed per minute	`G94 F200`
G95	Feed per revolution	`G95 F0.010`
G96	Constant surface speed	`G96 S400`
G97	Cancel CSS / direct RPM mode	`G97 S1500`
G98	Return to initial Z level	`G98`
G99	Return to R plane	`G99`

M-Codes (Miscellaneous)

Code	Description
M00	Program stop (unconditional)
M01	Optional stop
M02	End program
M03	Spindle on — clockwise
M04	Spindle on — counter-clockwise
M05	Spindle stop
M06	Tool change
M07	Mist coolant on
M08	Flood coolant on
M09	Coolant off
M10	Clamp
M11	Unclamp
M19	Spindle orient
M30	End program and rewind
M48	Enable feed/speed override
M49	Disable feed/speed override
M98	Call subprogram
M99	Return from subprogram

Address Codes

Letter	Meaning
A	Rotary axis A
B	Rotary axis B
C	Rotary axis C
D	Tool diameter offset number
F	Feed rate
G	Preparatory function
H	Tool length offset number
I	Arc center offset in X
J	Arc center offset in Y
K	Arc center offset in Z
L	Loop count / repetitions
M	Miscellaneous function
N	Line (sequence) number
O	Program number
P	Dwell time / subprogram number
Q	Peck depth (drilling cycles)
R	Arc radius / retract plane
S	Spindle speed
T	Tool number
X	X-axis position
Y	Y-axis position
Z	Z-axis position

Common Programming Patterns

Simple Face Milling Pass

G90 G54 G00 X0 Y0       (Absolute mode, WCS 1, rapid to start)
G43 H1 Z1.0             (Tool length comp, approach Z)
M03 S3000               (Spindle on CW at 3000 RPM)
G01 Z-0.050 F20.0       (Feed down to depth of cut)
G01 X6.0                (Feed across workpiece)
G00 Z1.0                (Rapid retract)
M05                     (Spindle stop)
G28 G91 Z0              (Return home Z)
M30                     (End program)

Peck Drilling

G90 G54 G00 X1.0 Y1.0   (Position over hole)
G43 H2 Z1.0             (Tool length comp)
M03 S2500               (Spindle on)
G83 X1.0 Y1.0 Z-1.0 R0.1 Q0.15 F5.0
                         (Peck drill: 0.15" pecks to -1.0" depth)
G80                     (Cancel canned cycle)
G00 Z1.0                (Retract)
M05
M30

Circular Interpolation (Arc)

G90 G54 G17              (Absolute, WCS 1, XY plane)
G00 X0 Y-0.5             (Rapid to arc start)
G43 H3 Z0.1
M03 S4000
G01 Z-0.125 F15.0        (Feed to depth)
G02 X0 Y-0.5 I0 J0.5 F12.0
                          (Full circle CW, center at 0, 0)
G00 Z1.0
M05
M30

Lathe-Specific G-Codes

Code	Description
G70	Finish cycle
G71	Rough turning cycle
G72	Rough facing cycle
G73	Pattern repeat cycle
G74	Peck drilling cycle (Z-axis)
G75	Grooving cycle (X-axis)
G76	Threading cycle (multi-pass)
G92	Threading cycle (single pass)
G96	Constant surface speed (CSS)
G97	Direct RPM mode

Disclaimer

The content on this page is provided for educational and quick-reference purposes only. It is not a substitute for manufacturer specifications, tooling documentation, or professional machining guidance. Always verify feeds, speeds, and tooling recommendations for your specific setup, machine, and material before machining. machref.com makes no warranty regarding the accuracy or completeness of this information. See our Terms of Service, Privacy Policy, and Accessibility Statement.