1. M Code Quick Reference Table

Code Description

M0 M1

Program Pause

M2 M30

Program End

M30 M60

Program Pause

M60

Program End

M3 M4 M5

Spindle Control

M6

Tool Change

M7 M8 M9

Coolant Control

M48

Feed & Spindle Overrides Enabled

M49

Feed & Spindle Overrides Disabled

M50

Feed Override Control

M51

Spindle Override Control

M52

Adaptive Feed Control

M53

Feed Stop Control

M61

Set Current Tool Number

M62-65

Output Control

M66

Input Control

M67

Analog Output Control

M68

Analog Output Control

M100-M199

User Defined M codes

2. 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 cycle start 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 cycle start button will restart the program at the following line.

Note
 It is OK to program M0 and M1 in MDI mode, but the effect will probably not be noticeable, because normal behavior in MDI mode is to stop after each line of input anyway.

3. M2, M30 Program End

  • M2 - end the program. Pressing cycle start 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:

  1. Change from Auto mode to MDI mode.

  2. Origin offsets are set to the default (like G54).

  3. Selected plane is set to XY plane (like G17).

  4. Distance mode is set to absolute mode (like G90).

  5. Feed rate mode is set to units per minute (like G94).

  6. Feed and speed overrides are set to ON (like M48).

  7. Cutter compensation is turned off (like G40).

  8. The spindle is stopped (like M5).

  9. The current motion mode is set to feed (like G1).

  10. Coolant is turned off (like M9).

Note
 Lines of code after M2/M30 will not be executed. Pressing cycle start will start the program at the beginning of the file.

4. M60 Program 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.

5. M3, M4, M5 Spindle Control

  • M3 - start the spindle clockwise at the S speed.

  • M4 - start the spindle counterclockwise at the S speed.

  • M5 - stop the spindle.

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.

6. M6 Tool Change

6.1. 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) Section.

6.2. 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), 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. The T number is an integer giving the changer slot of the tool (not its id).

  • 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 in its changer slot.

  • If configured in the .ini file some axis positions may move when a M6 is issued. See the EMCIO section of the Integrator’s Manual 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.

Warning
 The tool length offset is not changed by M6, use G43 after the M6 to change the tool length offset.

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.

7. M7, M8, M9 Coolant Control

  • M7 - turn mist coolant on.

  • M8 - turn flood coolant on.

  • M9 - turn all coolant off.

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

8. M48, M49 Override Control

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

  • M49 - disable both controls.

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

9. 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).

10. M51 Spindle Speed Override Control

  • M51 <P1> - enable the spindle speed override control. 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 Section).

11. 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).

12. 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.

13. M61 Set Current Tool Number

  • 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

14. M62 to M65 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 Integrator’s Manual Configuration Section LinuxCNC and HAL 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.

15. 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 (wait for digital input 0 to turn on)
M66 E1 L1 (wait for analog input 1 to rise)

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 Integrator’s Manual, Core Components Section, Motion subsection, for more information.

16. M67 Synchronized Analog Output

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 Integrator’s Manual, Core Components Section, Motion subsection, for more information.

17. M68 Analog Output

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 Integrator’s Manual, Core Components Section, Motion subsection, for more information.

18. M100 to 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.

The external program M1nn must be in the directory named in [DISPLAY] PROGRAM_PREFIX in the ini file and is executed with the P and Q values as its two arguments. Execution of the RS274/NGC file pauses until the invoked program exits. Any valid executable file can be used.

Warning
 Do not use a word processor to create or edit the files. A word processor will leave unseen codes that will cause problems and may prevent a bash or python file from working. Use a text editor like Gedit in Ubuntu or Notepad++ in other operating systems to create or edit the files.

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

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