M-Code Reference by Controller (Haas, LinuxCNC, GRBL, Marlin)

M-codes are machine functions that do not command axis motion. The core set is the same on most CNC controls: M00 program stop, M01 optional stop, M03 / M04 / M05 spindle clockwise / counter-clockwise / stop (speed in rpm from the S word), M06 tool change, M08 coolant on, M09 coolant off and M30 program end and reset. Beyond that the controls differ: Grbl has no M6 tool change and ignores M1; Haas uses M07 for shower coolant; and on Marlin 3D printers M30 deletes a file from the SD card while M104/M109 set the hotend temperature instead of working a probe arm, as they do on a Haas mill. Below: the four controls side by side, then the full Haas mill and lathe, LinuxCNC and Grbl lists from each maker's documentation. To see what a program's M-codes do line by line, paste it into the G-code Explainer & Simulator.

Core M-codes (Haas and LinuxCNC agree)

Numbers that go with M-codes

Same code, four controllers

Where the controls differ

• M6 tool change. Haas: M06 stops the spindle and coolant (including through-spindle coolant), moves Z to the tool-change position and orients the spindle by itself, so the program does not need M05, M09 or M19 first. LinuxCNC: the spindle stops, but "coolant will continue to flow during the tool change unless it has been turned off by an M9", and M6 does not change the tool length offset, so follow it with G43. With hal_manualtoolchange loaded, LinuxCNC stops and prompts the operator. Grbl rejects M6 with error:20. Marlin selects tools and extruders with T0–T7.
• M8 / M9 coolant. On LinuxCNC and Grbl, M7 and M8 can both be on and M9 turns both off. On a Haas mill M07 is the optional shower coolant; M09 stops shower and standard coolant; and with the Variable Flow Coolant option, M08 P0 / P1 / P2 run the pump at 50 / 60 / 80 Hz (low, normal, high pressure). Through-spindle coolant is M88 / M89 on Haas mills.
• M30 vs M2. Haas M30 stops the program, spindle and coolant (including TSC) and returns the cursor to the start; since Haas software 100.16.000.1041 it no longer cancels tool length offsets. LinuxCNC M2 and M30 both switch to MDI and reset work offset (G54), plane (G17), distance (G90), feed mode (G94), overrides (M48), cutter comp (G40), spindle (M5), motion (G1) and coolant (M9); M30 also exchanges pallet shuttles, and lines after either are not run. Grbl M2 and M30 reset G1, G17, G90, G94, G54, M5 and M9 but keep F, S and T. Marlin M30 deletes a named file from the SD card.
• M1 optional stop. Grbl accepts M1 and ignores it (its source says "Optional stop not supported"). Marlin documents M1 as a deprecated alias of M0, and both are ignored without an LCD or the emergency parser.
• M19 orient. Haas: P is whole degrees 0–360, R allows two decimals (M19 R123.45); a negative value orients to 0°. LinuxCNC: M19 R- Q- [P-], where R is the angle 0–360°, Q the seconds to wait for orientation, and P the direction (0 shortest, 1 clockwise, 2 counter-clockwise); it needs a spindle encoder.
• One M-code per line. Haas allows one M-code per block and runs it at the end of the block. LinuxCNC allows up to four M words per line from different modal groups, and runs them in a fixed order (M6 before M3, before M7–M9, before the stop codes M0/M1/M2/M30/M60), not in the order written.
• Codes above M99. LinuxCNC reserves M100–M199 for user-defined commands (scripts). Haas uses numbers above 100 for options (M104/M105 probe arm, M130 media display, M138/M139 spindle speed variation). Marlin uses them for printer functions (M104 hotend, M106 fan, M140 bed, M500 save settings). The same number can therefore do very different things.

Haas mill M-codes (full list)

Haas lathe M-codes (full list)

Mill vs lathe on the same make

• The Haas lathe list has no M06 and no M07; M10 / M11 are the chuck on a lathe but the 4th-axis brake on a mill; M12 / M13 are an air blast on a lathe but the 5th-axis brake on a mill; through-spindle coolant is M88 / M89 on a mill but M388 / M389 on a lathe, where M88 / M89 are high-pressure coolant.
• Spindle speed variation is M138 / M139 on both, and the lathe also lists M38 / M39 for it.

LinuxCNC M-codes

Grbl 1.1 M-codes

Marlin (3D printers): the M-codes that clash with CNC

• Marlin uses M-codes mostly for printer functions: M104 / M109 hotend temperature (set / set and wait), M140 / M190 bed temperature, M106 / M107 fan, M82 / M83 absolute / relative extrusion, M84 steppers off, M500 / M501 / M502 / M503 save / load / reset / report settings. The full list with parameters is on the Marlin G-code and M-code reference.
• M3 / M4 / M5 run a spindle or laser only when Marlin is built with spindle/laser support; M7 / M8 / M9 only with COOLANT_CONTROL. Without those build options they are not available.
• M30 is "Delete SD file" and M48 is a Z-probe repeatability test, so CNC programs must not be sent to a printer unchanged.

Program end on each control

(Haas mill, from Haas's own G81 example)
G00 G90 Z1. M09     (Rapid retract, coolant off)
G53 G49 Z0 M05      (Z home, spindle off)
G53 Y0              (Y home)
M30                 (End program)
%

(LinuxCNC, from its G80 example)
G80                 (turn off canned cycle)
G0 X0               (rapid move home)
M2                  (program end)

(Grbl)
M5
M9
M30

Sources

• Haas Automation, Mill Operator's Manual — 18: Mill M-Codes and Lathe Operator's Manual — Lathe M-Codes (haascnc.com/service/online-operator-s-manuals/…), with the Haas code pages for M00, M01, M02, M03–M05, M06, M07, M08/M09, M19, M29, M30, M97, M98 and M99. haascnc.com blocks automated downloads, so the pages were read from Internet Archive copies captured between July 2024 and August 2025 (web.archive.org). Used for: both Haas lists, the one-M-code-per-block rule, M06, M07, M08 P0–P2, M19, M30 and subprogram details.
• LinuxCNC Project, M-Codes and G-code Overview (modal groups, order of execution), linuxcnc.org/docs/html/gcode/m-code.html and …/overview.html, pages last updated 13 September 2026. Used for: the LinuxCNC list, modal groups, M2/M30 reset list, M6, M7–M9, M19, the four-M-words rule.
• gnea/grbl, Grbl 1.1h source (grbl/gcode.c) and README "List of Supported G-Codes in Grbl v1.1" (github.com/gnea/grbl), 2019. Used for: the Grbl list, M1 ignored, M2/M30 reset, M9 behaviour, unsupported M-codes.
• MarlinFirmware, Marlin G-code index (marlinfw.org/docs/gcode, source github.com/MarlinFirmware/MarlinDocumentation, downloaded 6 October 2026): pages for M0–M1, M3, M5, M7–M9, M30, M48, M104, M109. Used for: the Marlin column.
• All sources were read on 6 October 2026. Fanuc's own manuals are not freely published, so "Fanuc-style" behaviour on this page is taken from Haas's documentation only; check your machine builder's manual for other controls.