G-Code and M-Code List [ Easy To Use Examples & Tutorials ]

Complete CNC g code list with m-codes for milling in the Fanuc, LinuxCNC, GRBL, and Haas CNC machines dialects. We give a quick definition for all g codes along with a link to tutorials and examples of how to use it in CNC programming. Click the g-code link (if any) to visit a tutorial from our popuplar Online Free G-Code Training that shows examples and teaches how to program CNC machines using the g-code commands. This page is your ideal g-code reference.

G Codes and CNC G-Code List

Code	Category	Function	Notes
G00	Motion	g00 rapid: Move in a straight line at rapids speed.	XYZ of endpoint
G01	Motion	Move in a straight line at last speed commanded by a (F)eedrate	XYZ of endpoint
G02	Motion	Circular Interpolation: Clockwise circular arc at (F)eedrate	XYZ of endpoint IJK relative to center R for radius
G03	Motion	Circular Interpolation: Counter-clockwise circular arc at (F)eedrate	XYZ of endpoint IJK relative to center R for radius
G04	Motion	Dwell: Stop for a specified time.	P for milliseconds X for seconds
G05	Motion	FADAL Non-Modal Rapids
G09	Motion	Exact stop check

G10	Compensation	Programmable parameter input
G15	Coordinate	Turn Polar Coordinates OFF, return to Cartesian Coordinates
G16	Coordinate	Turn Polar Coordinates ON
G17	Coordinate	Select X-Y plane (Plane Selection)
G18	Coordinate	Select X-Z plane (Plane Selection)
G19	Coordinate	Select Y-Z plane (Plane Selection)
G20	Coordinate	Program coordinates are inches
G21	Coordinate	Program coordinates are mm
G27	Motion	Reference point return check
G28	Motion	Return to home position
G29	Motion	Return from the reference position
G30	Motion	Return to the 2nd, 3rd, and 4th reference point
G32	Canned	Constant lead threading (like G01 synchronized with spindle)
G40	Compensation	Tool cutter compensation off (radius comp.)
G41	Compensation	Tool cutter compensation left (radius comp.)
G42	Compensation	Tool cutter compensation right (radius comp.)
G43	Compensation	Apply tool length compensation (plus)
G44	Compensation	Apply tool length compensation (minus)
G49	Compensation	Tool length compensation cancel
G50	Compensation	Reset all scale factors to 1.0
G51	Compensation	Turn on scale factors
G52	Coordinate	Local workshift for all coordinate systems: add XYZ offsets
G53	Coordinate	Machine coordinate system (cancel work offsets)
G54	Coordinate	Work coordinate system (1st Workpiece)
G55	Coordinate	Work coordinate system (2nd Workpiece)
G56	Coordinate	Work coordinate system (3rd Workpiece)
G57	Coordinate	Work coordinate system (4th Workpiece)
G58	Coordinate	Work coordinate system (5th Workpiece)
G59	Coordinate	Work coordinate system (6th Workpiece)
G61	Other	Exact stop check mode
G62	Other	Automatic corner override
G63	Other	Tapping mode
G64	Other	Best speed path
G65	Other	Custom macro simple call
G68	Coordinate	Coordinate System Rotation
G69	Coordinate	Cancel Coordinate System Rotation
G73	Canned	High speed drilling cycle (small retract)
G74	Canned	Left hand tapping cycle
G76	Canned	Fine boring cyle
G80	Canned	Cancel canned cycle
G81	Canned	Simple drilling cycle
G82	Canned	Drilling cycle with dwell (counterboring)
G83	Canned	Peck drilling cycle (full retract)
G84	Canned	Tapping cycle
G85	Canned	Boring cycle, no dwell, feed out
G86	Canned	Boring cycle, spindle stop, rapid out
G87	Canned	Back boring canned cycle
G88	Canned	Boring canned cycle, spindle stop, manual out
G89	Canned	Boring canned cycle, dwell, feed out
G90	Coordinate	Absolute programming of XYZ (type B and C systems)
G90.1	Coordinate	Absolute programming IJK (type B and C systems)
G91	Coordinate	Incremental programming of XYZ (type B and C systems)
G91.1	Coordinate	Incremental programming IJK (type B and C systems)
G92	Coordinate	Offset coordinate system and save parameters
G92 (alternate)	Motion	Clamp of maximum spindle speed	S
G92.1	Coordinate	Cancel offset and zero parameters
G92.2	Coordinate	Cancel offset and retain parameters
G92.3	Coordinate	Offset coordinate system with saved parameters
G93	Motion	Inverse Time Feed Mode. For use with rotary axes
G94	Motion	Units per minute feed mode. Units in inches or mm.
G95	Motion	Units per revolution feed mode. Units in inches or mm.
G96	Motion	Constant surface speed
G97	Motion	Cancel constant surface speed
G98	Canned	Return to initial Z plane after canned cycle
G99	Canned	Return to initial R plane after canned cycle

M Code List to Control Machine Functions
	M Codes	Category	Function	Notes
	M00	M-Code	m00 Program Stop (non-optional)
	M01	M-Code	Optional Stop: Operator Selected to Enable
	M02	M-Code	End of Program
	M03	M-Code	m03 Spindle ON clockwise
	M04	M-Code	Spindle ON (CCW Rotation)
	M05	M-Code	m05 Spindle Stop
	M06	M-Code	Tool Change
	M07	M-Code	Mist Coolant ON
	M08	M-Code	Flood Coolant ON
	M09	M-Code	Coolant OFF

	M17	M-Code	FADAL subroutine return
	M29	M-Code	Rigid Tapping Mode on Fanuc Controls
	M30	M-Code	End of Program, Rewind and Reset Modes

	M97	M-Code	Haas-Style Subprogram Call
	M98	M-Code	Subprogram Call
	M99	M-Code	Return from Subprogram
	F	M-Code	Set Feedrate
	S	M-Code	Set Spindle Speed
	T	M-Code	Select Tool for Tool Change
	X, Y, Z, and A	M-Code	Sets coordinates for the axes: x axis, y axis, z axis and a axis.

Some Thoughts on G and M Codes

G and M Codes are the basic programming language used by most CNC Machines. These same g codes are probably the ones used by your CNC machine.

Most cnc programming of G and M codes is done using Computer Aided Manufacturing (CAM) Software. If you are able to program directly in G and M codes, you can do things that CAM software cannot. These things will make you a more productive CNC’er. Being able to control cnc machines at this level is one thing that can give machine shops competitive advantage.

Bonus: Check Out our Other CNC Cookbooks for More In-Depth CNC Information!

If you’re a CNC Beginnner, check out our CNC Beginner’s Cookbook. It’ll get you up to speed with a solid CNC foundation fast.

We also have Cookbooks for Feeds and Speeds, G-Code Programming, CNC Manufacturing and Shop Management, DIY CNC, and don’t forget the CNC Cookbook Blog–with over 4 million visitors a year it’s the most popular CNC blog by far on the web.

More Resources

Mazatrol Training Classes

Fanuc CNC Training Classes

G Code Commands FAQ

How many G codes are there in cnc machining?

There are about 100 g code commands, give or take. There are may dialects of g-code, and some have proprietary g-codes.

What are G Codes in CNC Machines?

This page lists all the G code commands used in CNC programming and tells what they do. It also gives links to tutorials and examples. G codes are single-letter commands that tell the CNC machine what to do. They may command motion (i.e. tell the machine where to cut) or do things like turn the spindle on or off.

Is learning G-Code hard?

Learning g-code isn't very hard. We have a complete free online g-code tutorial to teach you and a g-code simulator that makes learning easy.

Why are G Codes used?

G Codes make CNC Machines programmable, which gives them the flexibility to make almost any part.

What is the difference between G codes and M codes?

The G in G-Codes stands for Geometry, which means giving the CNC Machine directions on how and where to move. The four simplest motion-related g codes are:

G00: Move at the machine's fastest speed in a straight line to the commanded coordinates.
G01: Move at the last commanded feedrate (commanded by the "F" word) in a straight line to the commanded coordinates.
G02: Move in a clockwise arc to the commanded coordinates at the last commanded feedrate.
G03: Move in a counterclockwise arc to the commanded coordinates at the last commanded feedrate.

M Codes are about Machine functions on the CNC machine.

Do all CNC machines use G-code?

Not all CNC machines use G-Code. Some CNC machines may have both g-code and other ways of programming, for example, alternate languages such as Mazak's Mazatrol or Conversational Programming. Others may have an alternate language and no ability to execute g-code at all.

Recently updated on June 12th, 2024 at 08:05 am