CNC M Code List: Functions and Common Uses

An M code (miscellaneous code) is a CNC program command used to control machine functions beyond axis motion. G codes define motion and machining modes, while M codes commonly control spindle operation, coolant, tool changes, and program flow. The same M-code number can have different functions depending on the controller and machine configuration.

Some M codes are common across CNC machines, while others depend on the controller or machine model. The list below covers common M codes and their typical functions.

For a broader explanation of how G codes and M codes work together in a CNC program, see the guide to G code and M code in CNC programming.

CNC M Code List and Their Functions

This CNC M code list combines commonly used commands with documented machine-specific assignments for CNC milling and turning. The codes are organized numerically for quick reference. When the same code has different functions across controls or machine types, each assignment is listed separately.

The common-code descriptions represent widely used conventions, not a universal standard. Machine-specific examples are identified by control or machine type. Refer to the Haas mill M-code list, Haas lathe M-code list, and LinuxCNC M-code reference for the documented implementations shown below. Always verify the exact code definition, machine options, and execution requirements before running a program.

The table covers frequently used commands and a broad range of documented control-specific assignments, but it does not replace the complete programming manual for a particular machine. Additional M codes may be available for options such as automatic part loading, tool probing, custom relays, or machine-builder-specific automation.

When two controls assign different meanings to the same M code, use the row for the exact controller and machine configuration. Do not transfer a code definition from one machine to another based on the number alone.

CNC machine and control panel displaying M codes

How Do M Codes Differ Between CNC Milling and Turning?

Many commonly used M codes serve the same basic purpose on milling and turning machines. For example, M03/M04/M05 are commonly used for spindle control, while M08/M09 control coolant on supported machines. Exact implementation still depends on the control and machine builder.

The differences are specific to one machine type. Turning centers may include chuck, tailstock, bar-feeder, and subspindle functions. The available M codes depend on the machine's equipment and control configuration.

Chuck and tailstock commands are machine-specific. On Haas lathes, M10/M11 clamp and unclamp the chuck, while M21/M22 advance and retract the tailstock. Do not infer these functions from the code number alone when working with another machine. On a turning center with a subspindle for second-operation machining, M codes control which spindle is active, whether parts transfer between spindles, and how the subspindle synchronizes with the main spindle during part handoff.

Live-tool turning centers use separate commands for the main spindle and the live-tool spindle. On Haas lathes, M133 starts the live tool forward, M134 runs it in reverse, and M135 stops the live tool. M12/M13 control the optional auto jet air blast, while M14/M15 control the main-spindle brake on supported C-axis configurations. Other machine builders may assign different codes, so verify which spindle each command controls in the machine manual.

Pallet-change commands depend on the control and automation package. Haas mills use M50 for the pallet-change sequence. LinuxCNC documents M60 as a pallet-change pause. Whether an actual pallet exchange occurs depends on the configured hardware, external logic, and machine implementation. The two commands are not interchangeable. Follow the sequence specified for the target machine.

Treat common spindle and coolant M codes as a starting reference, not proof of full program compatibility. Before running a program on a specific machine, verify any M code that controls auxiliary hardware and confirm its execution sequence against the machine builder's documentation.

Example of M Codes in a CNC Program

The following simplified CNC milling program illustrates common M-code sequencing on a Fanuc-style vertical machining center with an automatic tool changer and flood coolant. It assumes that tool T02 has a matching H02 tool-length offset and that G54 Z0 is set at the top of the workpiece. The programmed Z50.0 position must provide adequate clearance for the actual setup. M-code behavior and tool-change sequences vary by machine, so verify the program against the target machine's programming manual before use.

O2001                        ; Program number
N010 G21 G17 G40 G49 G80 G94 ; Set metric units, XY plane, and feed per minute; cancel cutter comp, tool length comp, and canned cycles
N020 G28 G91 Z0              ; Return Z to machine reference using incremental mode
N030 G90 G54                 ; Absolute mode and work coordinate system
N040 T02 M06                 ; Load tool 2 (12 mm end mill; confirm H02 matches its measured length)
N050 S3500 M03               ; Set spindle speed and start spindle clockwise
N060 G00 X0 Y0               ; Rapid to XY start position; confirm Z clearance is safe
N070 G43 H02 Z50.0           ; Apply tool length offset H02 and move to safe Z
N080 M08                     ; Flood coolant on
N090 G00 Z5.0                ; Rapid to 5 mm above the workpiece
N100 G01 Z-10.0 F150         ; Feed to cutting depth at 150 mm/min
N110 X80.0 F400              ; Linear cut at 400 mm/min
N120 Y50.0                   ; Continue cutting in Y
N130 X0                      ; Return in X
N140 Y0                      ; Return in Y
N150 G00 Z50.0               ; Retract to safe height
N160 M09                     ; Coolant off
N170 M05                     ; Spindle stop
N180 G49                     ; Cancel tool length compensation
N190 G28 G91 Z0              ; Return Z to machine reference
N200 M30                     ; End program and rewind/reset as supported

M-code sequencing affects how the machine executes the program. In this example, coolant starts before the first cutting move and turns off after the tool retracts. The spindle starts before cutting begins and stops after machining is complete. In a multi-tool program, check whether the machine stops the spindle automatically during M06; if not, program M05 before the tool change as required by the machine builder.

For an inspection pause, insert M00 at the intended stop point rather than replacing M30. M00 pauses program execution, while spindle and coolant behavior depends on the machine. After inspection, follow the controller's restart procedure before continuing.

How to Verify M Code Compatibility Before Running a CNC Program

Running a CNC program with unverified M codes is a direct path to unexpected machine behavior. The verification process has four components.

1. Check the machine builder's programming manual

   This is the authoritative source for M code definitions on a specific machine. The manual lists every M code the machine implements, what it does, any prerequisites (machine must be at home, spindle must be stopped), and whether the code has options or parameters. Documentation from major machine builders such as Haas, Mazak, DMG MORI, and Okuma is often available online; older machines may require a physical manual.

2. Check the CNC controller documentation

   The controller and the machine builder are sometimes different entities. A machine built by one manufacturer running a Fanuc 31i controller will have both machine-builder-specific M codes and Fanuc-standard M codes. Both documentation sources are needed to understand the full M code behavior on that specific machine.

3. Verify the CAM post-processor configuration

   CAM software outputs M codes based on the post-processor selected for the target machine. A generic post-processor produces generic M codes that may not match the specific machine. The post-processor should be configured for the exact machine and controller combination, including correct M code numbers for tool change, coolant, and any machine-specific functions used. A post-processor configured for a different machine can output M codes that do not match the target machine. Here's a guide to CNC post-processors explaining how CAM output is converted into code for a specific machine and controller.

4. Simulate and prove out the program before cutting

   CNC simulation can check tool motion and the M-code behavior supported by its machine model. It may not reproduce every machine-specific auxiliary function, particularly when the control or post-processor has not been configured to represent that hardware. Before the first production run on a new program or machine, follow the machine builder's prove-out procedure. Where appropriate, use graphics mode or a controlled dry run with rapid override reduced and the tool clear of the workpiece. Confirm that the spindle and coolant respond as programmed, and verify the actual tool-change sequence before machining material. Investigate any unexpected behavior before the cutting run.

Precision CNC Machining Service

Upload your CAD file to get a fast quote starting from $1, with lead times as short as 3 days.

Get Instant Quote

FAQs About CNC M Codes