Discrete ManufacturingFree referencePDF, Excel, Word exportMachine Shops

CNC G-Code Reference Table

A G-code lookup is one of the most searched machining references. This table lists the codes used daily on mills and lathes with a plain-language function and the traps that usually catch people.

Download:

G-code	Function	Group	Mill / Lathe	Notes
G00	Rapid positioning	Motion	Both	Non-cutting move at maximum traverse. Check the path for clamps and the part.
G01	Linear interpolation	Motion	Both	Straight cutting move at the programmed F feed.
G02	Circular interpolation clockwise	Motion	Both	Use I, J, K center offsets or an R radius.
G03	Circular interpolation counterclockwise	Motion	Both	Same address words as G02.
G04	Dwell	Non-modal	Both	Pause using P (milliseconds on many controls) or X (seconds). Check your control.
G09	Exact stop, single block	Non-modal	Both	Decelerates to exact position at the end of the block.
G10	Programmable data input	Non-modal	Both	Writes work or tool offsets from the program.
G17	XY plane selection	Plane	Mill	Default plane for arcs and cutter compensation on most mills.
G18	ZX plane selection	Plane	Both	Default plane on a lathe.
G19	YZ plane selection	Plane	Mill	For arcs in the YZ plane.
G20	Inch units	Units	Both	Fanuc-style. Some controls use G70 for inch.
G21	Metric units	Units	Both	Fanuc-style. Some controls use G71 for metric.
G28	Return to machine home via intermediate point	Non-modal	Both	Usually used with G91 for a safe move to zero return.
G30	Return to second reference point	Non-modal	Both	Commonly used for tool change position.
G40	Cutter radius compensation cancel	Compensation	Mill	Cancel on a move away from the part.
G41	Cutter compensation left	Compensation	Mill	Uses a D word to select the radius offset.
G42	Cutter compensation right	Compensation	Mill	Climb vs conventional depends on spindle direction and side.
G43	Tool length compensation, positive	Compensation	Mill	Uses an H word and Z move to activate.
G49	Tool length compensation cancel	Compensation	Mill	Cancels G43 and G44.
G52	Local coordinate system shift	Non-modal	Both	Temporary shift of the work coordinate system. Cancel with G52 X0 Y0 Z0.
G53	Machine coordinate system move	Non-modal	Both	Applies to the current block only.
G54	Work coordinate system 1	Work offset	Both	G54 to G59 select the first six work offsets.
G55	Work coordinate system 2	Work offset	Both	Often used for the second fixture position.
G56	Work coordinate system 3	Work offset	Both	Same family as G54.
G57	Work coordinate system 4	Work offset	Both	Same family as G54.
G58	Work coordinate system 5	Work offset	Both	Same family as G54.
G59	Work coordinate system 6	Work offset	Both	Further offsets use G54.1 P or G110 and up, depending on control.
G61	Exact stop mode	Path mode	Mill	Decelerates at every corner. Cancel with G64.
G64	Cutting (blending) mode	Path mode	Mill	Smoother motion without stopping at each block end.
G68	Coordinate system rotation	Transform	Mill	Rotates the program about a point. Cancel with G69.
G69	Coordinate rotation cancel	Transform	Mill	Cancels G68.
G73	High speed peck drilling cycle	Canned cycle	Mill	Short retract between pecks to break chips.
G76	Fine boring cycle (mill)	Canned cycle	Mill	Stops spindle and shifts the tool off the wall before retracting. On a lathe G76 is a threading cycle.
G80	Canned cycle cancel	Canned cycle	Both	Always cancel before the next unrelated move.
G81	Drilling cycle	Canned cycle	Mill	Feed in, rapid out.
G82	Drilling cycle with dwell	Canned cycle	Mill	Dwell at the bottom for spot facing or counterbores.
G83	Peck drilling cycle	Canned cycle	Mill	Full retract between pecks to clear chips. Deep holes.
G84	Tapping cycle, right hand	Canned cycle	Mill	Needs a tap holder or rigid tapping (M29 on many Fanuc-style controls).
G85	Boring cycle, feed in and feed out	Canned cycle	Mill	Spindle keeps turning on retract.
G90	Absolute programming	Distance mode	Mill	Coordinates are relative to the work zero. On many lathes G90 is a turning cycle.
G91	Incremental programming	Distance mode	Mill	Coordinates are relative to the current position.
G92	Set position / thread cycle	Setting	Both	Mill: sets a position register. Some lathe controls use G92 for threading.
G94	Feed per minute	Feed mode	Mill	F is in inches or mm per minute.
G95	Feed per revolution	Feed mode	Both	F is in inches or mm per spindle revolution.
G96	Constant surface speed	Spindle mode	Lathe	S is surface speed. Set a G50 limit first to cap RPM.
G97	Direct RPM	Spindle mode	Lathe	S is spindle RPM. Cancels constant surface speed.
G98	Return to initial level after canned cycle	Canned cycle	Mill	Retracts to the Z level before the cycle started.
G99	Return to R plane after canned cycle	Canned cycle	Mill	Retracts only to the R plane; faster between holes.
G50	Spindle speed limit / coordinate setting	Setting	Lathe	Used with S to cap RPM under G96 on Fanuc-style lathes.
G70	Finishing cycle	Turning cycle	Lathe	Finish pass along the profile defined for G71 or G72.
G71	Rough turning cycle (stock removal)	Turning cycle	Lathe	Roughs along Z using a profile defined by blocks.

Codes shown follow common Fanuc-style conventions. Haas, Siemens, Heidenhain, Mazak and others differ in details, and G-code groups, G70 to G72 and cycle formats vary by control. Always check the programming manual for your machine before running a program.

Govern CNC programs alongside ERP routings

Optional: we can discuss linking program revisions and approvals to routings and part masters.

Optional. The tool and every export work without this. No spam.

How to use the table

Type a code, function or keyword in the search box to filter the table, for example G83, tapping, or compensation. Each row gives the code, what it does, its group, whether it applies to a mill, a lathe or both, and a note about behavior or cautions. Export the table to Excel or PDF if you want a printed cheat sheet for the machine. Because controls differ, use it as a quick reminder, then confirm the exact format in your machine's manual.

Modal and non-modal codes

Most G-codes are modal: they stay active until another code in the same group replaces them. G01, G90, G17 and G54 all remain in effect across blocks. Non-modal codes such as G04, G28 or G53 apply only to the line they appear on. This is why a safe start-up line usually restates the modal states, for example G90 G54 G17 G40 G49 G80, so a program does not inherit the previous job's state.

Motion: G00, G01, G02, G03 (one active at a time)
Distance mode: G90 or G91
Work offset: G54 to G59 and extended offsets
Canned cycles stay active until G80

Controls differ

There is no single universal G-code standard. ISO 6983 defines a common core, but each builder adds extensions. G20 and G21 select units on Fanuc-style controls while older controls use G70 and G71. G90 is absolute positioning on a mill but a turning cycle on some lathe controls. G76 means a fine boring cycle on a mill and a threading cycle on a lathe. Siemens and Heidenhain use their own languages with different cycle calls. Read the manual for your specific control.

Common mistakes

Forgetting G80 after a canned cycle can cause unexpected drilling on the next move. Leaving cutter compensation active through a rapid can gouge a part. Mixing G90 and G91 without a restatement is a classic source of crashes. On lathes, running G96 without a G50 RPM cap can send the spindle to its maximum when the tool approaches the centerline. Always dry run or single block a new program with feed and rapid overrides lowered.

Frequently Asked Questions

What is the difference between G00 and G01?

G00 is a rapid, non-cutting move at the machine's traverse speed. G01 is a linear move at the programmed feed rate, used for cutting. Using G00 into material or G01 for long air moves are both common mistakes.

What does G54 do?

G54 selects work coordinate system 1, which maps program coordinates to a position on the machine set by the operator during setup. G55 to G59 select further work offsets so multiple fixtures or parts can share one program.

Are G-codes the same on every CNC machine?

No. A core set is shared, but details differ by control builder and machine type. Cycle formats, canned cycle parameters and even unit codes change. Use this table as a refresher and check the manual for your control before relying on a code.

What does it mean when a G-code is modal?

A modal code remains active until another code from the same group is programmed. For example, once G01 is active it applies to following moves until G00, G02 or G03 replaces it. Non-modal codes apply only to their own block.

If CNC programs, revisions and approvals are managed by file shares rather than your ERP or PLM, Netray can help connect them to part and routing records with read-only controls.

Talk to an Expert Explore More Free Tools

Related Tools

Discrete Manufacturing

More Discrete Manufacturing tools

See all

Back to All Tools