CNC programming reference

Common G-codes and M-codes, explained.

A practical reference for the CNC commands machinists use most—from motion and work offsets to canned cycles, spindle control, and coolant.

G01

Linear interpolation

G01 X2.000 Y1.000 F20.0

See Helio machine monitoring

Controller behavior varies. This reference covers common Fanuc-style mill programming conventions, but codes and parameters can differ across Haas, Siemens, Heidenhain, Mazak, Okuma, LinuxCNC, and machine-builder implementations. Verify every program against your machine manual, simulate it, and use safe prove-out procedures.

G-codes define the path

They set motion, planes, units, offsets, compensation, and machining cycles.

M-codes control the machine

They handle spindle, coolant, tool changes, stops, and program flow.

Many G-codes are modal: once called, they remain active until another command in the same group replaces or cancels them. A safe program start explicitly sets the critical modes instead of assuming what the previous program left active.

Motion codes

Swipe the table to see descriptions →

Code	Function	What it does
`G00`	Rapid positioning	Moves one or more axes at the machine's rapid rate. Normally used for non-cutting moves.
`G01`	Linear interpolation	Moves in a straight line at the programmed feed rate.
`G02`	Clockwise arc	Cuts a clockwise circular or helical move in the active plane.
`G03`	Counterclockwise arc	Cuts a counterclockwise circular or helical move in the active plane.
`G04`	Dwell	Pauses motion for a programmed amount of time.Note: The P address may represent milliseconds, seconds, or a decimal value depending on the control.

Setup and coordinate codes

Swipe the table to see descriptions →

Code	Function	What it does
`G17`	XY plane selection	Selects the XY plane for arcs, cutter compensation, and some canned cycles.
`G18`	ZX plane selection	Selects the ZX plane.
`G19`	YZ plane selection	Selects the YZ plane.
`G20`	Inch units	Interprets programmed dimensions in inches.
`G21`	Metric units	Interprets programmed dimensions in millimeters.
`G28`	Return to reference position	Returns an axis to machine reference through an intermediate point.Note: An unintended intermediate move can cause a collision; many shops prefer an explicit G53 move.
`G53`	Machine coordinates	Makes the move in the machine coordinate system rather than the active work offset.
`G54–G59`	Work coordinate offsets	Selects one of the standard work coordinate systems.
`G90`	Absolute positioning	Positions are measured from the active work-coordinate origin.
`G91`	Incremental positioning	Each position is measured from the current location.
`G94`	Feed per minute	Programs feed as distance traveled per minute.
`G95`	Feed per revolution	Programs feed as distance traveled per spindle revolution.

Tool compensation

Swipe the table to see descriptions →

Code	Function	What it does
`G40`	Cancel cutter compensation	Cancels G41 or G42 cutter-radius compensation.
`G41`	Cutter compensation left	Offsets the toolpath to the left of the programmed contour, viewed in the direction of travel.
`G42`	Cutter compensation right	Offsets the toolpath to the right of the programmed contour, viewed in the direction of travel.
`G43`	Tool-length compensation	Applies the selected positive tool-length offset, commonly with an H address.
`G49`	Cancel tool-length compensation	Cancels the active tool-length compensation.

Common canned cycles

Swipe the table to see descriptions →

Code	Function	What it does
`G80`	Cancel canned cycle	Cancels the active drilling, tapping, or boring cycle.
`G81`	Drilling cycle	Feeds to depth and rapids out without a dwell.
`G82`	Drilling with dwell	Feeds to depth, dwells, and then rapids out.
`G83`	Peck drilling cycle	Drills in repeated pecks to help clear chips from a deep hole.
`G84`	Tapping cycle	Coordinates spindle direction and axial feed for tapping.
`G85`	Boring cycle	Feeds into and out of the hole without stopping the spindle.

Common M-codes

Swipe the table to see descriptions →

Code	Function	What it does
`M00`	Program stop	Stops the program until the operator restarts it.
`M01`	Optional stop	Stops only when Optional Stop is enabled on the control.
`M03`	Spindle clockwise	Starts the spindle clockwise at the programmed S speed.
`M04`	Spindle counterclockwise	Starts the spindle counterclockwise at the programmed S speed.
`M05`	Spindle stop	Stops spindle rotation.
`M06`	Tool change	Commands an automatic tool change on equipped machines.
`M07`	Mist coolant on	Turns on mist or auxiliary coolant when supported.
`M08`	Flood coolant on	Turns on flood coolant.
`M09`	Coolant off	Turns off active coolant outputs.
`M19`	Spindle orientation	Orients the spindle to a fixed angular position when supported.
`M30`	Program end and reset	Ends the program, resets it, and commonly rewinds to the beginning.
`M98`	Call subprogram	Calls a subprogram, often using P for the program number and L for repeat count.
`M99`	Return from subprogram	Returns from a subprogram; behavior in a main program varies by control.

A complete program example

This simple inch-mode milling example selects Tool 1, activates the G54 work offset, applies tool-length compensation, makes one feed move, and returns the Z axis in machine coordinates before ending.

%
O1001 (SIMPLE LINEAR CUT)
G20 G17 G40 G49 G80 G90
T01 M06
G54
S2500 M03
G00 X0.000 Y0.000
G43 H01 Z0.100
M08
G01 Z-0.125 F8.0
G01 X2.000 F20.0
G00 Z0.500
M09
M05
G53 G00 Z0.
M30
%

This is an instructional example, not a ready-to-run production program. Tooling, workholding, offsets, clearances, feeds, speeds, and controller behavior must be validated for the actual machine.

What G-code cannot tell you

G-code describes what the controller was asked to do. It does not prove what happened at the machine. The program alone cannot show that a tool dulled halfway through a run, spindle load drifted upward, a cycle waited on an operator, or the machine sat idle between jobs.

The useful distinction

G-code controls the machine. Helio shows what the machine actually did.

Connect cycle time, spindle load, alarms, utilization, and operator context to see where production diverges from the plan.

Frequently asked questions

Are G-codes the same on every CNC machine?

No. Core motion commands such as G00, G01, G02, and G03 are broadly shared, but syntax, canned cycles, parameters, and machine-specific M-codes vary by controller and machine builder. Always verify a program against the exact machine manual.

What is the difference between a G-code and an M-code?

G-codes generally define geometry, motion, units, coordinate systems, and machining cycles. M-codes generally control machine functions such as the spindle, coolant, tool changes, stops, and subprogram flow.

What does modal mean in G-code?

A modal command stays active until another command in the same modal group replaces or cancels it. For example, G01 remains active for subsequent coordinate blocks until another motion mode such as G00, G02, or G03 is programmed.

Controller documentation

Use this page as a quick reference, then confirm syntax in the official documentation for your control. Useful starting points include the Haas mill G-code list, Haas mill M-code list, and the LinuxCNC G-code documentation.