m-code.rst

M Codes
=======

M Code Quick Reference Table
----------------------------

================================ =======================================
Code                             Description
================================ =======================================
`M0 M1 <#mcode:m0-m1>`__         Program Pause
`M2 M30 <#mcode:m2-m30>`__       Program End
`M60 <#mcode:m60>`__             Pallet Change Pause
`M3 M4 M5 <#mcode:m3-m4-m5>`__   Spindle Control
`M6 <#mcode:m6>`__               Tool Change
`M7 M8 M9 <#mcode:m7-m8-m9>`__   Coolant Control
`M19 <#mcode:m19>`__             Orient Spindle
`M48 M49 <#mcode:m48-m49>`__     Feed & Spindle Overrides Enable/Disable
`M50 <#mcode:m50>`__             Feed Override Control
`M51 <#mcode:m51>`__             Spindle Override Control
`M52 <#mcode:m52>`__             Adaptive Feed Control
`M53 <#mcode:m53>`__             Feed Stop Control
`M61 <#mcode:m61>`__             Set Current Tool Number
`m62-m65 <#mcode:m62-m65>`__     Output Control
`M66 <#mcode:m66>`__             Input Control
`M67 <#mcode:m67>`__             Analog Output Control
`M68 <#mcode:m68>`__             Analog Output Control
`M70 <#mcode:m70>`__             Save Modal State
`M71 <#mcode:m71>`__             Invalidate Stored Modal State
`M72 <#mcode:m72>`__             Restore Modal State
`M73 <#mcode:m73>`__             Save Autorestore Modal State
`M98 M99 <#mcode:m98-m99>`__     Call and Return From Subprogram
`M100-M199 <#mcode:m100-m199>`__ User Defined M-Codes
================================ =======================================

M0, M1 Program Pause
--------------------

* 'M0' - pause a running program temporarily. LinuxCNC remains in the Auto Mode so MDI and other
   manual actions are not enabled. Pressing the resume button will restart the program at the
   following line.
* 'M1' - pause a running program temporarily if the optional stop switch is on. LinuxCNC remains in
   the Auto Mode so MDI and other manual actions are not enabled. Pressing the resume button will
   restart the program at the following line.

[TABLE]

M2, M30 Program End
-------------------

* 'M2' - end the program. Pressing r will start the program at the beginning of the file.
* 'M30' - exchange pallet shuttles and end the program. Pressing cycle start will start the program
   at the beginning of the file.

Both of these commands have the following effects:

#. Change from Auto mode to MDI mode.
#. Origin offsets are set to the default (like 'G54').
#. Selected plane is set to XY plane (like 'G17').
#. Distance mode is set to absolute mode (like 'G90').
#. Feed rate mode is set to units per minute (like 'G94').
#. Feed and speed overrides are set to ON (like 'M48').
#. Cutter compensation is turned off (like 'G40').
#. The spindle is stopped (like 'M5').
#. The current motion mode is set to feed (like 'G1').
#. Coolant is turned off (like 'M9').

M60 Pallet Change Pause
-----------------------

* 'M60' - exchange pallet shuttles and then pause a running program temporarily (regardless of the
   setting of the optional stop switch).  Pressing the cycle start button will restart the program
   at the following line.

M3, M4, M5 Spindle Control
--------------------------

* 'M3' - start the selected spindle clockwise at the 'S' speed.
* 'M4' - start the selected spindle counterclockwise at the 'S' speed.
* 'M5' - stop the selected spindle.

Use $ to operate on specific spindles. If $ is omitted then thr commands operate on all spindles.

For example

.. code:: highlight

   ---
   S100 $0
   S200 $1
   S300 $2
   M3
   ----
   Will start all three spindles simultaneously at different speeds
   [source,{ngc]]
   ----
   M4 $1
   ----
   Will then reverse spindle 1 but leave the other spindles rotating forwards.

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 <#sec:set-spindle-speed>`__ 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.

M6 Tool Change
--------------

Manual Tool Change
~~~~~~~~~~~~~~~~~~

If the HAL component hal_manualtoolchange is loaded, M6 will stop the spindle and prompt the user to
change the tool based on the last 'T-' number programmed. For more information on
hal_manualtoolchange see the `Manual Tool Change <#sec:manual-tool-change>`__ section.

Tool Changer
~~~~~~~~~~~~

To change a tool in the spindle from the tool currently in the spindle to the tool most recently
selected (using a T word - see Section `Select Tool <#sec:select-tool>`__), program 'M6'. When the
tool change is complete:

* The spindle will be stopped.

* The tool that was selected (by a T word on the same line or on any line after the previous tool
  change) will be in the spindle.

* If the selected tool was not in the spindle before the tool change, the tool that was in the
  spindle (if there was one) will be placed back into the tool changer magazine.

* If configured in the .ini file some axis positions may move when a M6 is issued. See the `EMCIO
  section <#sec:emcio-section>`__ for more information on tool change options.

* No other changes will be made. For example, coolant will continue to flow during the tool change
   unless it has been turned off by an 'M9'.

The tool change may include axis motion. It is OK (but not useful) to program a change to the tool
already in the spindle. It is OK if there is no tool in the selected slot; in that case, the spindle
will be empty after the tool change. If slot zero was last selected, there will definitely be no
tool in the spindle after a tool change. The tool changer will have to be setup to perform the tool
change in hal and possibly classicladder.

M7, M8, M9 Coolant Control
--------------------------

-  'M7' - turn mist coolant on. M7 controls iocontrol.0.coolant-mist
   pin.

-  'M8' - turn flood coolant on. M8 controls iocontrol.0.coolant-flood
   pin.

-  'M9' - turn both M7 and M8 off.

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 Orient Spindle
------------------

-  'M19 R- Q- [P-] [$-]'

-  'R' Position to rotate to from 0, valid range is 0-360 degrees

-  'Q' Number of seconds to wait until orient completes. If
   spindle.N.is-oriented does not become true within Q timeout an error
   occurs.

-  'P' Direction to rotate to position.

   -  '0' rotate for smallest angular movement (default)

   -  '1' always rotate clockwise (same as M3 direction)

   -  '2' always rotate counterclockwise (same as M4 direction)

-  '$' The spindle to orient (actually only determines which HAL pins
   carry the spindle position commands)

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.

ORIENT_OFFSET = 0-360 (fixed offset in degrees added to M19 R word)

HAL Pins

-  'spindle.N.orient-angle' (out float) Desired spindle orientation for
   M19. Value of the M19 R word parameter plus the value of the
   [RS274NGC]ORIENT_OFFSET ini parameter.

-  'spindle.N.orient-mode' (out s32) Desired spindle rotation mode.
   Reflects M19 P parameter word, Default = 0

-  'spindle.N.orient' (out bit) Indicates start of spindle orient cycle.
   Set by M19. Cleared by any of M3,M4,M5. If spindle-orient-fault is
   not zero during spindle-orient true, the M19 command fails with an
   error message.

-  'spindle.N.is-oriented' (in bit) Acknowledge pin for spindle-orient.
   Completes orient cycle. If spindle-orient was true when
   spindle-is-oriented was asserted, the spindle-orient pin is cleared
   and the spindle-locked pin is asserted. Also, the spindle-brake pin
   is asserted.

-  'spindle.N.orient-fault' (in s32) Fault code input for orient cycle.
   Any value other than zero will cause the orient cycle to abort.

-  'spindle.N.locked' (out bit) Spindle orient complete pin. Cleared by
   any of M3,M4,M5.

M48, M49 Speed and Feed Override Control
----------------------------------------

-  'M48' - enable the spindle speed and feed rate override controls.

-  'M49' - disable both controls.

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 <#sub:feed-rate>`__ Section for more
details.

M50 Feed Override Control
-------------------------

-  'M50 <P1>' - enable the feed rate override control. The P1 is
   optional.

-  'M50 P0' - disable the feed rate control.

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).

M51 Spindle Speed Override Control
----------------------------------

-  'M51 <P1> <$→'- enable the spindle speed override control for the
   selected spindle. The P1 is optional.

-  'M51 P0 <$→' - disable the spindle speed override control program.
   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 `Spindle Speed <#sec:set-spindle-speed>`__
   Section).

M52 Adaptive Feed Control
-------------------------

-  'M52 <P1>' - use an adaptive feed. The P1 is optional.

-  'M52 P0' - stop using adaptive feed.

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. Values on
'motion.adaptive-feed' should range from 0 (feed hold) to 1 (full
speed).

M53 Feed Stop Control
---------------------

-  'M53 <P1>' - enable the feed stop switch. The P1 is optional.
   Enabling the feed stop switch will allow motion to be interrupted by
   means of the feed stop control. In LinuxCNC, the HAL pin
   'motion.feed-hold' is used for this purpose. A 'true' value will
   cause the motion to stop when 'M53' is active.

-  'M53 P0' - disable the feed stop switch. The state of
   'motion.feed-hold' will have no effect on feed when M53 is not
   active.

M61 Set Current Tool
--------------------

-  'M61 Q-' - change the current tool number while in MDI or Manual
   mode. One use is when you power up LinuxCNC with a tool currently in
   the spindle you can set that tool number without doing a tool change.

It is an error if:

-  Q- is not 0 or greater

M62 - M65 Digital Output Control
--------------------------------

-  'M62 P-' - turn on digital output synchronized with motion. The P-
   word specifies the digital output number.

-  'M63 P-' - turn off digital output synchronized with motion. The P-
   word specifies the digital output number.

-  'M64 P-' - turn on digital output immediately. The P- word specifies
   the digital output number.

-  'M65 P-' - turn off digital output immediately. 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 <#sec:motion>`__
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.

[TABLE]

M66 Wait on Input
-----------------

::

   M66 P- | E- <L->

-  'P-' - specifies the digital input number from 0 to 3.

-  'E-' - specifies the analog input number from 0 to 3.

-  'L-' - specifies the wait mode type.

   -  'Mode 0: IMMEDIATE' - no waiting, returns immediately. The current
      value of the input is stored in parameter #5399

   -  'Mode 1: RISE' - waits for the selected input to perform a rise
      event.

   -  'Mode 2: FALL' - waits for the selected input to perform a fall
      event.

   -  'Mode 3: HIGH' - waits for the selected input to go to the HIGH
      state.

   -  'Mode 4: LOW' - waits for the selected input to go to the LOW
      state.

-  'Q-' - specifies the timeout in seconds for waiting. If the timeout
   is exceeded, the wait is interrupt, and the variable #5399 will be
   holding the value -1. The Q value is ignored if the L-word is zero
   (IMMEDIATE). A Q value of zero is an error if the L-word is non-zero.

-  Mode 0 is the only one permitted for an analog input.

M66 Example Lines

::

   M66 P0 L3 Q5 (wait up to 5 seconds for digital input 0 to turn on)

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 <#sec:motion>`__ for more information.

[TABLE]

Example HAL Connection

::

   net signal-name motion.digital-in-00 <= parport.0.pin10-in

M67 Analog Output,Synchronized
------------------------------

::

   M67 E- Q-

-  'M67' - set an analog output synchronized with motion.

-  'E-' - output number ranging from 0 to 3.

-  'Q-' - is the value to set (set to 0 to turn off).

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 <#sec:motion>`__ for more information.

[TABLE]

M68 Analog Output, Immediate
----------------------------

::

   M68 E- Q-

-  'M68' - set an analog output immediately.

-  'E-' - output number ranging from 0 to 3.

-  'Q-' - is the value to set (set to 0 to turn off).

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 <#sec:motion>`__ for more information.

[TABLE]

M70 Save Modal State
--------------------

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 inadvertant modal changes within subroutines.

The state saved consists of:

-  current G20/G21 settings (imperial/metric)

-  selected plane (G17/G18/G19 G17.1,G18.1,G19.1)

-  status of cutter compensation (G40,G41,G42,G41.1,G42,1)

-  distance mode - relative/absolute (G90/G91)

-  feed mode (G93/G94,G95)

-  current coordinate system (G54-G59.3)

-  tool length compensation status (G43,G43.1,G49)

-  retract mode (G98,G99)

-  spindle mode (G96-css or G97-RPM)

-  arc distance mode (G90.1, G91.1)

-  lathe radius/diameter mode (G7,G8)

-  path control mode (G61, G61.1, G64)

-  current feed and speed ('F' and 'S' values)

-  spindle status (M3,M4,M5) - on/off and direction

-  mist (M7) and flood (M8) status

-  speed override (M51) and feed override (M50) settings

-  adaptive feed setting (M52)

-  feed hold setting (M53)

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

'current call level' means either:

-  executing in the main program. There is a single storage location for
   state at the main program level; if several 'M70' instructions are
   executed in turn, only the most recently saved state is restored when
   an 'M72' is executed.

-  executing within a G-code subroutine. The state saved with 'M70'
   within a subroutine behaves exactly like a local named parameter - it
   can be referred to only within this subroutine invocation with an
   'M72' and when the subroutine exits, the parameter goes away.

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

M71 Invalidate Stored Modal State
---------------------------------

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.

M72 Restore Modal State
-----------------------

`Modal state saved with an 'M70' <#mcode:m70-saved-state>`__ 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 explicitely 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:

.. code:: highlight

   O<showstate> sub
   (DEBUG, imperial=#<_imperial> absolute=#<_absolute> feed=#<_feed> rpm=#<_rpm>)
   O<showstate> endsub

   O<imperialsub> sub
   g20 (imperial)
   g91 (relative mode)
   F5 (low feed)
   S300 (low rpm)
   (debug, in subroutine, state now:)
   o<showstate> call
   O<imperialsub> endsub

   ; main program
   g21 (metric)
   g90 (absolute)
   f200 (fast speed)
   S2500 (high rpm)

   (debug, in main, state now:)
   o<showstate> call

   M70 (save caller state in at global level)
   O<imperialsub> call
   M72 (explicitely restore state)

   (debug, back in main, state now:)
   o<showstate> call
   m2

M73 Save and Autorestore Modal State
------------------------------------

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 inadvertant modal changes. Note the use of `predefined named
parameters <#gcode:predefined-named-parameters>`__ in the 'showstate'
subroutine.

.. code:: highlight

   O<showstate> sub
   (DEBUG, imperial=#<_imperial> absolute=#<_absolute> feed=#<_feed> rpm=#<_rpm>)
   O<showstate> endsub

   O<imperialsub> sub
   M73 (save caller state in current call context, restore on return or endsub)
   g20 (imperial)
   g91 (relative mode)
   F5 (low feed)
   S300 (low rpm)
   (debug, in subroutine, state now:)
   o<showstate> call

   ; note - no M72 is needed here - the following endsub or an
   ; explicit 'return' will restore caller state
   O<imperialsub> endsub

   ; main program
   g21 (metric)
   g90 (absolute)
   f200 (fast speed)
   S2500 (high rpm)
   (debug, in main, state now:)
   o<showstate> call
   o<imperialsub> call
   (debug, back in main, state now:)
   o<showstate> call
   m2

M98 and M99
-----------

The interpreter supports Fanuc-style main- and sub-programs with the
'M98' and 'M99' M-codes. See `Fanuc-Style
Programs <#ocode:fanuc-style-programs>`__.

Selectively Restoring Modal State
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

Executing an 'M72' or returning from a subroutine which contains an
'M73' will restore `all modal state saved <#mcode:m70-saved-state>`__.

If only some aspects of modal state should be preserved, an alternative
is the usage of `predefined named
parameters <#gcode:predefined-named-parameters>`__, local parameters and
conditional statements. The idea is to remember the modes to be restored
at the beginning of the subroutine, and restore these before exiting.
Here is an example, based on snippet of
'nc_files/tool-length-probe.ngc':

.. code:: highlight

   O<measure> sub   (measure reference tool)
   ;
   #<absolute> = #<_absolute>  (remember in local variable if G90 was set)
   ;
   g30 (above switch)
   g38.2 z0 f15 (measure)
   g91 g0z.2 (off the switch)
   #1000=#5063 (save reference tool length)
   (print,reference length is #1000)
   ;
   O<restore_abs> if [#<absolute>]
       g90 (restore G90 only if it was set on entry:)
   O<restore_abs> endif
   ;
   O<measure> endsub

M100 - M199 User Defined Commands
---------------------------------

::

   M1-- <P- Q->

-  'M1--' - an integer in the range of 100 - 199.

-  'P-' - a number passed to the file as the first parameter.

-  'Q-' - a number passed to the file as the second parameter.

[TABLE]

The external program named 'M100' through 'M199' (no extension and a
capitol M) 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 specificed in the ini file configuration. See
the `Display Section <#sec:display-section>`__ for more information on
search paths.

[TABLE]

The error 'Unknown M code used' denotes one of the following

-  The specified User Defined Command does not exist

-  The file is not an executable file

-  The file name has an extension

-  The file name does not follow this format M1nn where nn = 00 through
   99

-  The file name used a lower case M

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.

M101 Example File

::

   #!/bin/bash
   # file to turn on parport pin 14 to open the collet closer
   halcmd setp parport.0.pin-14-out True
   exit 0

M102 Example File

::

   #!/bin/bash
   # file to turn off parport pin 14 to open the collet closer
   halcmd setp parport.0.pin-14-out False
   exit 0

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

::

   M100 P123.456 Q321.654

M100 Example file

::

   #!/bin/bash
   voltage=$1
   feedrate=$2
   halcmd setp thc.voltage $voltage
   halcmd setp thc.feedrate $feedrate
   exit 0

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.

M110 Example file

::

   #!/bin/bash
   eog /home/john/linuxcnc/nc_files/message.png
   exit 0

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

M110 Example display and keep going

::

   #!/bin/bash
   eog /home/john/linuxcnc/nc_files/message.png &
   exit 0

Last updated 2018-12-26 02:40:49 CET