FANUC Machine Code Quick Reference

This guide is a quick reference for common address codes and instructions in FANUC CNC programs. Before programming a real machine, check the machine manufacturer's manual, system parameters, and site safety procedures. Some M codes and macro functions are customized by machine builders.

G Codes (Preparatory Functions)

G codes define preparatory machining functions such as motion, coordinate modes, units, compensation, and canned cycles. Most G codes are modal: they remain active until replaced by another code in the same group.

Code	Meaning	Example / Notes
G00	Rapid positioning	G00 X100. Y50.: move the tool rapidly to the specified position
G01	Linear interpolation	G01 Z-5. F100: cut in a straight line to Z-5. at the programmed feed
G02	Clockwise circular interpolation	G02 X50. Y0 I25. J0: machine a clockwise arc
G03	Counterclockwise circular interpolation	G03 X50. Y0 R25.: machine a counterclockwise arc with radius 25
G04	Dwell	G04 P1000: pause for about 1 second (units depend on system parameters)
G09	Exact stop check	G09 G01 X50.: decelerate and stop precisely before the block ends
G10	Programmable data input	G10 L2 P1 X0 Y0 Z0: write work coordinate system data
G17	Select XY plane	Common for milling, drilling, and XY-plane circular interpolation
G18	Select ZX plane	Common for turning or ZX-plane circular interpolation
G19	Select YZ plane	Common for YZ-plane circular interpolation
G20	Inch units	G20: interpret subsequent dimensions in inches
G21	Metric units	G21: interpret subsequent dimensions in millimeters
G27	Reference position check	Check whether the current position is the reference position
G28	Return to reference position	G91 G28 Z0: return the Z axis to machine reference via an intermediate point
G29	Return from reference position	Usually used with G28
G30	Return to second/third/fourth reference position	G30 P2 Z0: return to the specified reference position, often for tool changes
G31	Skip function / probing skip	Often used for probe measurements or skip-signal triggers
G40	Cancel cutter radius compensation	G40 G01 X0 Y0: move after canceling compensation
G41	Cutter radius compensation left	Compensate to the left of the cutting direction; requires a D offset number
G42	Cutter radius compensation right	Compensate to the right of the cutting direction; requires a D offset number
G43	Positive tool length compensation	G43 H01 Z50.: enable H01 tool length compensation
G44	Negative tool length compensation	Less common; apply tool length compensation in the negative direction
G49	Cancel tool length compensation	G49: cancel the active length compensation
G50	Coordinate system / spindle speed limit setting	Lathes commonly use G50 S3000 to limit maximum spindle speed
G52	Local coordinate system setting	G52 X10. Y0: temporarily offset the local coordinate system
G53	Machine-coordinate positioning	G53 G00 Z0: rapid positioning in machine coordinates
G54	Work coordinate system 1	G54: select the first work coordinate system
G55	Work coordinate system 2	G55: select the second work coordinate system
G56	Work coordinate system 3	G56: select the third work coordinate system
G57	Work coordinate system 4	G57: select the fourth work coordinate system
G58	Work coordinate system 5	G58: select the fifth work coordinate system
G59	Work coordinate system 6	G59: select the sixth work coordinate system
G61	Exact stop mode	Check for an exact stop at the end of every machining block
G64	Cutting / continuous cutting mode	Run smoothly between blocks where possible, reducing pauses
G65	Macro call	G65 P9000 A10. B20.: call macro program O9000
G66	Modal macro call	Call the specified macro on subsequent blocks until canceled by G67
G67	Cancel modal macro call	G67: cancel the G66 modal macro call
G68	Coordinate rotation	G68 X0 Y0 R45.: rotate coordinates around the specified point
G69	Cancel coordinate rotation	G69: cancel the active coordinate rotation
G73	High-speed peck drilling cycle	G73 X0 Y0 Z-20. Q2. F100: deep drilling with short retracts
G74	Left-hand / reverse tapping cycle	Confirm the exact function for the machine model and parameters
G76	Fine boring / threading cycle	Usually fine boring on machining centers; often a compound threading cycle on lathes
G80	Cancel canned cycle	G80: cancel drilling, tapping, boring, and other canned cycles
G81	Drilling cycle	G81 X0 Y0 Z-10. R2. F100: standard drilling
G82	Drilling cycle with dwell	G82 X0 Y0 Z-10. R2. P500 F100: dwell at the bottom of the hole
G83	Deep-hole drilling cycle	G83 X0 Y0 Z-30. R2. Q5. F80: peck drilling for chip removal
G84	Tapping cycle	G84 X0 Y0 Z-15. R2. F1.5: right-hand tapping
G85	Boring cycle	Feed in and feed out
G86	Boring cycle	Stop the spindle at the bottom, then retract rapidly
G87	Back boring cycle	Often used for reverse boring; verify machine support
G88	Boring cycle	Dwell and stop the spindle at the bottom; retract manually or by the specified method
G89	Boring cycle	Feed out after a dwell at the bottom
G90	Absolute coordinate programming	G90 G00 X100.: target an absolute position in the coordinate system
G91	Incremental coordinate programming	G91 G00 X10.: move 10 relative to the current position
G92	Coordinate system setting / threading cycle	Meaning varies by system and turning/milling application; check the manual
G94	Feed per minute	G94 F200: feed at 200 mm/min
G95	Feed per revolution	G95 F0.2: feed 0.2 mm/rev of the spindle
G96	Constant surface speed	Common on lathes: G96 S180 sets 180 m/min
G97	Cancel constant surface speed / fixed RPM	G97 S1200: set a fixed spindle speed of 1200 rpm
G98	Canned cycle return to initial point	Return to the initial plane at the start of the cycle
G99	Canned cycle return to R point	Return to the R plane at the end of the cycle

M Codes (Auxiliary Functions)

M codes control auxiliary actions such as spindle rotation, coolant, tool changes, program stops, and clamping. Machine builders often extend or redefine M codes; follow the machine manual on site.

Code	Meaning	Example / Notes
M00	Program stop	Stop unconditionally; resume with Cycle Start
M01	Optional stop	Stop only when the panel's optional stop switch is enabled
M02	End program	End the program, usually without rewinding to its beginning
M03	Spindle forward	S1200 M03: rotate forward at 1200 rpm
M04	Spindle reverse	S800 M04: rotate in reverse at 800 rpm
M05	Spindle stop	Stop the current spindle rotation
M06	Automatic tool change	T01 M06: select tool 1 and change tools
M08	Coolant on	Start cutting fluid / coolant pump
M09	Coolant off	Stop coolant
M10	Clamp / lock	Often clamps a fixture, fourth axis, or chuck; machine-dependent
M11	Unclamp / unlock	Often releases a fixture, fourth axis, or chuck; machine-dependent
M13	Spindle forward and coolant on	Commonly equivalent to M03 + M08
M14	Spindle reverse and coolant on	Commonly equivalent to M04 + M08
M19	Spindle orientation	Orient before tool changes, boring retracts, or positioned machining
M30	End program and reset	End the program and usually return to its beginning
M48	Enable feed / spindle overrides	Allow override switches; confirm system parameters
M49	Disable feed / spindle overrides	Ignore override settings; confirm system parameters
M60	Pallet change	Common APC pallet exchange on machining centers; depends on configuration
M98	Subprogram call	M98 P1000 L2: call subprogram O1000 twice
M99	Subprogram return / loop	Return to the main program from a subprogram; may loop in a main program

T Codes (Tools)

T codes specify tool numbers, offset numbers, or initiate a tool change. Machining centers and lathes often use very different formats.

Code	Meaning	Example / Notes
T01	Select tool 1	Machining centers commonly use T01 M06 for an automatic tool change
T12	Select tool 12	T12 M06: call tool 12 from the magazine
T0101	Tool number + offset number	Common lathe format: first two digits select tool, last two select offset
T0100	Call tool and cancel offset	On lathes, commonly retains the tool number while canceling the offset
T0000	Cancel tool / offset	On lathes, commonly cancels the active tool compensation state

S Codes (Spindle)

S codes set spindle speed or a constant surface speed target, usually alongside M03, M04, G96, or G97.

Code	Meaning	Example / Notes
S1200	Set spindle speed	S1200 M03: spindle forward at a target 1200 rpm
S800	Set a lower speed	S800 M04: spindle reverse at a target 800 rpm
G97 S1500	Fixed RPM mode	Cancel constant surface speed and set spindle speed to 1500 rpm
G96 S180	Constant surface speed mode	Common on lathes; set surface speed to 180 m/min
G50 S3000	Maximum spindle speed limit	Limit top speed while turning at constant surface speed

F Codes (Feed)

F codes set cutting feed rates. Feed units depend on modes such as G94 and G95.

Code	Meaning	Example / Notes
F100	Set feed value	G01 Z-5. F100: feed at 100 in the current feed mode
G94 F200	Feed per minute	Common units: mm/min, e.g. 200 mm/min
G95 F0.2	Feed per revolution	Common units: mm/rev, e.g. 0.2 mm per spindle revolution
G01 X50. F150	Linear cutting feed	Used with cutting motions such as G01, G02, and G03
G00	Rapid motion is not controlled by F	Rapid positioning speed is normally controlled by machine parameters and overrides

Coordinate and Common Address Words

Address words provide coordinates, radii, offset numbers, cycle parameters, or macro arguments for G/M/T/S/F instructions.

Code	Meaning	Example / Notes
X	X-axis coordinate	X100.: move the X axis to or by 100
Y	Y-axis coordinate	Y50.: move the Y axis to or by 50
Z	Z-axis coordinate	Z-10.: move the Z axis to or by -10
A	A rotary axis	Usually a fourth axis rotating about X
B	B rotary axis	Usually rotates about Y
C	C rotary axis	Usually rotates about Z
U	Incremental X address	Common on lathes, indicating an X-direction increment
V	Incremental Y address	Indicates a Y-direction increment; availability depends on configuration
W	Incremental Z address	Common on lathes, indicating a Z-direction increment
I	Arc-center X offset	In G02 X50. Y0 I25. J0, I is the arc-center X offset
J	Arc-center Y offset	In G03 X0 Y50. I0 J25., J is the arc-center Y offset
K	Arc-center Z offset	Common for arcs in ZX/YZ planes
R	Arc radius / canned-cycle R point	G03 X50. Y0 R25.; R2. is the return plane for drilling
P	Dwell time / program number / parameter	G04 P1000; M98 P1000 calls a subprogram
Q	Depth per cut / peck amount	G83 Z-30. Q5.: drill 5 per peck
D	Cutter radius offset number	G41 D01: apply D01 radius offset
H	Tool length offset number	G43 H01 Z50.: apply H01 length offset
L	Repeat count / parameter selection	M98 P1000 L3: repeat subprogram 3 times
N	Block number	N100 G01 X50.: a block number helps locate code
O	Program number	O1000: define or call a numbered program

Common Combinations

Code	Meaning	Example / Notes
G21 G17 G40 G49 G80 G90	Safe machining-center initialization	Metric, XY plane, cancel radius/length offsets and cycles, absolute mode
G54 G00 X0 Y0	Select coordinates and position rapidly	Rapidly move to the work origin after selecting G54
T01 M06	Change to tool 1	Common machining-center tool-change format
S1200 M03	Spindle forward	Set 1200 rpm and start forward rotation
G43 H01 Z50.	Enable tool length compensation	Apply H01 and move to safe height Z50.
M08 / M09	Coolant on / off	Turn coolant on at the start of machining and off at the end
G91 G28 Z0	Z-axis return to reference	Often used to retract and home; beware of incremental-mode risks
M05 M30	Stop spindle and end program	Common combination at program end

Usage Notes

Code	Meaning	Example / Notes
G00	Rapid moves can cause collisions	Use single-block, dry run, and reduced override on the first run
G90 / G91	Confirm absolute / incremental mode	Especially important during homing, array machining, and macros
G54-G59	Verify work coordinate systems	Check zero, fixture, offsets, and program before machining
M codes	Often customized by builders	Consult the machine manual for clamping, chip removal, air blast, door locks, etc.
T / H / D	Match tools and offsets	Verify tool, length offset, and radius offset numbers against installed tools