M-Codes

Both of these commands have the following effects:

Use $ to operate on specific spindles. If $ is omitted then the commands default to operating on spindle 0. Use $-1 to operate on all active spindles.

This example will start spindles 0, 1, and 2 simultaneously at different speeds:

This example will then reverse spindle 1 but leave the other spindles rotating forwards:

And this will stop spindle 2 and leave the other spindles rotating:

If the $ is omitted then behaviour is exactly as normal for a single spindle machine.

It is OK to use M3 or M4 if the S spindle speed is set to zero. If this is done (or if the speed override switch is enabled and set to zero), the spindle will not start turning. If, later, the spindle speed is set above zero (or the override switch is turned up), the spindle will start turning. It is OK to use M3 or M4 when the spindle is already turning or to use M5 when the spindle is already stopped.

Connect one or both of the coolant control pins in HAL before M7 or M8 will control an output. M7 and M8 can be used to turn on any output via G-code.

It is OK to use any of these commands, regardless of the current coolant state.

M19 is a command of modal group 7, like M3, M4 and M5. M19 is cleared by any of M3,M4,M5.

Spindle orientation requires a quadrature encoder with an index to sense the spindle shaft position and direction of rotation.

INI Settings in the [RS274NGC] section:

These commands also take an optional $ parameter to determine which spindle they operate on.

It is OK to enable or disable the controls when they are already enabled or disabled. See the Feed Rate section for more details.

They also can be be toggled individually using M50 and M51, see below.

While disabled the feed override will have no influence, and the motion will be executed at programmed feed rate. (unless there is an adaptive feed rate override active).

While disabled the spindle speed override will have no influence, and the spindle speed will have the exact program specified value of the S-word (described in the Spindle Speed section).

When adaptive feed is enabled, some external input value is used together with the user interface feed override value and the commanded feed rate to set the actual feed rate. In LinuxCNC, the HAL pin motion.adaptive-feed is used for this purpose. The range for motion.adaptive-feed is defined by the MAX_FEED_OVERRIDE value in the [DISPLAY] section of the ini file and will be limited to a range of -MAX_FEED_OVERRIDE to MAX_FEED_OVERRIDE. 0 is equivalent to feed-hold.

It is an error if:

The P- word specifies the digital output number. The P-word ranges from 0 to a default value of 3. If needed the the number of I/O can be increased by using the num_dio parameter when loading the motion controller. See the Motion section for more information.

The M62 & M63 commands will be queued. Subsequent commands referring to the same output number will overwrite the older settings. More than one output change can be specified by issuing more than one M62/M63 command.

The actual change of the specified outputs will happen at the beginning of the next motion command. If there is no subsequent motion command, the queued output changes won’t happen. It’s best to always program a motion G-code (G0, G1, etc) right after the M62/63.

M64 & M65 happen immediately as they are received by the motion controller. They are not synchronized with movement, and they will break blending.

M66 wait on an input stops further execution of the program, until the selected event (or the programmed timeout) occurs.

It is an error to program M66 with both a P-word and an E-word (thus selecting both an analog and a digital input). In LinuxCNC these inputs are not monitored in real time and thus should not be used for timing-critical applications.

The number of I/O can be increased by using the num_dio or num_aio parameter when loading the motion controller. See the Motion section for more information.

The actual change of the specified outputs will happen at the beginning of the next motion command. If there is no subsequent motion command, the queued output changes won’t happen. It’s best to always program a motion G-code (G0, G1, etc) right after the M67. M67 functions the same as M62-63.

The number of I/O can be increased by using the num_dio or num_aio parameter when loading the motion controller. See the Motion section for more information.

M68 output happen immediately as they are received by the motion controller. They are not synchronized with movement, and they will break blending. M68 functions the same as M64-65.

The number of I/O can be increased by using the num_dio or num_aio parameter when loading the motion controller. See the Motion section for more information.

To explicitly save the modal state at the current call level, program M70. Once modal state has been saved with M70, it can be restored to exactly that state by executing an M72.

A pair of M70 and M72 instructions will typically be used to protect a program against inadvertent modal changes within subroutines.

The state saved consists of:

Note that in particular, the motion mode (G1 etc) is NOT restored.

current call level means either:

A recursive invocation of a subroutine introduces a new call level.

Modal state saved with an M70 or by an M73 at the current call level is invalidated (cannot be restored from anymore).

A subsequent M72 at the same call level will fail.

If executed in a subroutine which protects modal state by an M73, a subsequent return or endsub will not restore modal state.

The usefulness of this feature is dubious. It should not be relied upon as it might go away.

Modal state saved with an M70 code can be restored by executing an M72.

The handling of G20/G21 is specially treated as feeds are interpreted differently depending on G20/G21: if length units (mm/in) are about to be changed by the restore operation, 'M72 'will restore the distance mode first, and then all other state including feed to make sure the feed value is interpreted in the correct unit setting.

It is an error to execute an M72 with no previous M70 save operation at that level.

The following example demonstrates saving and explicitly restoring modal state around a subroutine call using M70 and M72. Note that the imperialsub subroutine is not "aware" of the M7x features and can be used unmodified:

To save modal state within a subroutine, and restore state on subroutine endsub or any return path, program M73.

Aborting a running program in a subroutine which has an M73 operation will not restore state .

Also, the normal end (M2) of a main program which contains an M73 will not restore state.

The suggested use is at the beginning of a O-word subroutine as in the following example. Using M73 this way enables designing subroutines which need to modify modal state but will protect the calling program against inadvertent modal changes. Note the use of predefined named parameters in the showstate subroutine.

The interpreter supports Fanuc-style main- and sub-programs with the M98 and M99 M-codes. See Fanuc-Style Programs.

The external program named M100 through M199 (no extension, a capital M, found in directory pointed by [DISPLAY] PROGRAM_PREFIX parameter of the INI file) is executed with the optional P and Q values as its two arguments.

Execution of the G-code file pauses until the external program exits. Any valid executable file can be used. The file must be located in the search path specified in the INI file configuration. See the Display section for more information on search paths.

After creating a new M1nn program, the GUI should be restarted so that the new program is taken into account, otherwise a Unknown M-code error will occur.

The error Unknown M-code used denotes one of the following:

For example to open and close a collet closer that is controlled by a parallel port pin using a bash script file using M101 and M102. Create two files named M101 and M102. Set them as executable files (typically right click/properties/permissions) before running LinuxCNC. Make sure the parallel port pin is not connected to anything in a HAL file.

To pass a variable to a M1nn file you use the P and Q option like this:

To display a graphic message and stop until the message window is closed use a graphic display program like Eye of Gnome to display the graphic file. When you close it the program will resume.

To display a graphic message and continue processing the G-code file suffix an ampersand to the command.