Discrete ManufacturingFree referencePDF, Excel, Word exportMachine Shops

CNC M-Code Reference Table

M-codes are the miscellaneous machine functions: spindle, coolant, tool change and program flow. This table lists the ones programmers use daily and flags the ones that change from machine to machine.

Download:

M-code	Function	Group	Mill / Lathe	Notes
M00	Program stop	Program control	Both	Stops until the operator presses cycle start. Spindle and coolant may stop depending on the control.
M01	Optional stop	Program control	Both	Stops only if the optional stop switch is on.
M02	End of program	Program control	Both	Ends the program. Does not always rewind.
M03	Spindle on, clockwise	Spindle	Both	Needs an S word. Normal for right-hand cutting tools.
M04	Spindle on, counterclockwise	Spindle	Both	For left-hand tools and some tapping setups.
M05	Spindle stop	Spindle	Both	Program before an operator interaction or a tool change on some controls.
M06	Tool change	Tool	Mill	Select the tool with T, then M06 to swap. Often preceded by a move to the tool change position.
M07	Mist coolant on	Coolant	Both	Option on many machines.
M08	Flood coolant on	Coolant	Both	Standard flood coolant.
M09	Coolant off	Coolant	Both	Turns off M07 and M08.
M10	Clamp / chuck or axis clamp (varies)	Machine option	Both	Meaning varies by builder. Check the manual.
M11	Unclamp (varies)	Machine option	Both	Meaning varies by builder.
M13	Spindle clockwise with coolant on	Spindle	Both	ISO combined code, not on all controls.
M14	Spindle counterclockwise with coolant on	Spindle	Both	ISO combined code, not on all controls.
M19	Spindle orient	Spindle	Both	Stops the spindle at a fixed angle. Used for boring bar shift and tool change.
M29	Rigid tapping mode	Spindle	Mill	Fanuc-style. Placed before G84 so spindle and Z are synchronized.
M30	End of program and rewind	Program control	Both	Resets the program to the start. Standard end of a program.
M41	Spindle low gear range	Spindle	Lathe	Gear range codes M41 to M44 on many Fanuc-style lathes.
M42	Spindle second gear range	Spindle	Lathe	Range depends on the machine.
M43	Spindle third gear range	Spindle	Lathe	Range depends on the machine.
M44	Spindle fourth gear range	Spindle	Lathe	Range depends on the machine.
M48	Enable feed and speed override	Override	Both	Allows operator overrides after M49.
M49	Disable feed and speed override	Override	Both	Common during threading or tapping on some controls.
M97	Local subprogram call (some controls)	Subprogram	Both	Haas-style call to a label in the same program.
M98	Subprogram call	Subprogram	Both	Call with P for program number, and L or Q for repeat count, depending on control.
M99	Subprogram return / program loop	Subprogram	Both	Returns to the calling program. At the end of a main program it can loop.

M-codes are defined mostly by the machine builder, not by a universal standard. Codes shown follow common Fanuc and Haas-style usage. Verify every code in your machine's documentation, especially M10 to M19 and options like through-spindle coolant, chip conveyors and pallet changers.

Link CNC program governance to ERP records

Optional: we can discuss how program revisions and machine-specific data could be tied to part and routing records.

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

How to use the table

Search by code or by function, for example M08, coolant or subprogram. Each row gives the function, its group, whether it applies to a mill, lathe or both, and a note on common behavior. Export it to Excel or PDF as a desk reference or to add machine-specific codes for your own shop. Because M-codes are largely set by the builder, add your machine's own columns for options like pallet change, parts catcher and through-spindle coolant.

Which M-codes are standard

A core group is nearly universal: M00 and M01 for stops, M02 and M30 for program end, M03, M04 and M05 for spindle, M06 for tool change, M08 and M09 for coolant, and M98 and M99 for subprograms. Beyond that the numbers are assigned by the control or machine builder. M10 and M11, for example, clamp and unclamp on some machines and mean other things on others. Machine builders also add numbered codes for options such as probes, pallets and bar feeders.

Program control: M00, M01, M02, M30
Spindle: M03, M04, M05, M19
Coolant: M07, M08, M09
Tool and subprograms: M06, M98, M99

M02 versus M30

Both end a program, but M30 also rewinds it to the first block so the next cycle start begins from the top, while M02 may stop at the end with the program pointer unchanged on some controls. Most shops standardize on M30 as the last line of every main program. M99 behaves differently: at the end of a subprogram it returns to the calling program, and at the end of a main program it can loop the program back to the start, which can be used for bar-fed production.

Common mistakes

A frequent crash cause is forgetting M05 or M09 before a manual operation, or calling M06 without moving to a safe position first. Another is relying on a code from one machine on another: M19 orientation, M29 rigid tapping and clamp codes all differ. Also remember that an M-code in a block with a motion command may execute before, with or after the move depending on the code and the control, so put critical spindle commands on their own lines.

Frequently Asked Questions

What is the difference between M02 and M30?

Both end the program. M30 ends it and returns to the beginning of the program so it is ready for the next part, while M02 simply ends it and may not rewind. Most shops use M30 on every main program.

What do M03, M04 and M05 do?

M03 starts the spindle clockwise, M04 starts it counterclockwise and M05 stops it. M03 and M04 need a spindle speed S word, either in the same block or earlier. Most right-hand cutting tools run under M03.

Are M-codes the same on all CNC machines?

Only the common ones. Stops, spindle, coolant and program end are widely consistent, but many M-codes are assigned by the machine builder for options and differ. Always check your machine's manual before using unfamiliar codes.

What does M98 do?

M98 calls a subprogram, using P for the program number and an optional repeat count depending on the control. The subprogram ends with M99 to return. It is used for repeated features, multiple parts on a fixture and long toolpath files.

If machine-specific code lists and post-processor settings live in individual programmers' heads, Netray can help capture them against machine and part records for governance.

Talk to an Expert Explore More Free Tools

Related Tools

Discrete Manufacturing

More Discrete Manufacturing tools

See all

Back to All Tools