en:software:mdurosettacncsoftwaregcode:supported_g_m-codes

1. Supported G and M Codes

The following table describes supported G-Code commands.
The G-codes and M-codes called in the same line of a G-code file are executed accordingly to G Code Order of Execution.

In the following axes means one or more of X, Y, Z, A, B, C, along with a corresponding floating-point value for a specified axis.

Gcode Parameters Command Description
G0 axes Straight traverse Traverse at maximum velocity.
G1 axes F Straight feed Move at feed rate F.
G2 axes F P IJK or R Clockwise arc feed Arc at feed rate F.
G3 axes F P IJK or R Counterclockwise arc feed Arc at feed rate F.
G4 P Dwell Pause for P seconds.
G9 axes F Exact Stop (non-modal) Move at feed rate F and stop at the end.
G10 L1 P axes Set Tool Table Entry

Update the tool table adding/updating the tool info with the tool offset set by the user.
Arguments: * P tool id * X tool offset X * Y tool offset Y * Z tool offset Z * D tool diameter * Q tool type * I tool parameter 1 * J tool parameter 2 * K tool parameter 3 * V tool slot: this should be specified only if the tool is not already present in the tool table.

G10 L10 P axes Set Tool Table, Calculated, Workpiece

Update the tool table adding/updating the tool info with the tool offset calculated by the G-code interpreter.
* P tool id * X the X position that should be considered 0 when the tool is loaded and tool offset are used * Y the Y position that should be considered 0 when the tool is loaded and tool offset are used * Z the Z position that should be considered 0 when the tool is loaded and tool offset are used * D tool diameter * Q tool type * I tool parameter 1 * J tool parameter 2 * K tool parameter 3 * V tool slot: this should be specified only if the tool is not already present in the tool table.

G10 L2 P axes Coordinate System Origin Setting

G10 L2 offsets the origin of the coordinate system specified by P to the value of the axis word.
The offset is from the machine origin established during homing.
The offset value will replace any current offsets in effect for the coordinate system specified. Axis words not used will not be changed.

G10 L20 P axes Coordinate Origin Setting Calculated G10 L20 is similar to G10 L2 except that instead of setting the WCS origin offset, it calculates and sets the values that makes the current coordinates corresponds to the specified arguments.
G10 L100 P<parameter> V<value> Set the value of some special parameters
G15 Switch to Cartesian coordinates
G16 Switch to polar coordinates
G17 Select XY arc plane
G18 Select XZ arc plane
G19 Select YZ arc plane
G20 Select inches mode All G-code from this point on will be interpreted in inches
G21 Select mm mode All G-code from this point on will be interpreted in millimetres
G28 axes Go to G28 position Optional axes specify an intermediate point
G28.1 Set G28 position Store the current machine position so that it will be used by G28
G30 axes Go to G30 position Optional axes specify an intermediate point
G30.1 Set G30 position Store the current machine position so that it will be used by G30
G38.2 G38.3 G38.4 G38.5 axes Probing
G40 Disable Cutter Compensation
G41 D I Enable Cutter Compensation left of programmed path
G41.1 D L Enable Dynamic Cutter Compensation left of programmed path
G42 D I Enable Cutter Compensation right of programmed path
G42.1 D L Enable Dynamic Cutter Compensation right of programmed path
G43 H Enable Tool Length Compensation H argument is optional, if it is not specified the current tool is used.
G43.1 X Y Z Enable Dynamic Tool Length Compensation Tool compensation is enabled considering the specified offsets X, Y and Z. The arguments X,Y and Z are optional but at least one should be specified.
G43.2 H Apply additional Tool Length Offset Add the offsets due to the tool specified with the H argument to the offsets already in use.
G43.4 H Enable RTCP feature Enable Rotation tool center point control. (See 1. RTCP)
G43.7 H <X> <Y> <Z> Enable RTCP feature and override tool offsets using user defined arguments
G49 Cancel Tool Length Compensation and disable RTCP feature
G50 Disable scaling
G51 X Y Z and I J K or P Enable scaling
G52 axes Local Work Shift The values entered are added to all work offsets
G53 Select absolute coordinates Non-Modal: Applies only to current block
G54 Select coord system 1 G54 is typically used as the “normal” coordinate system and reflects the machine position
G55 Select coord system 2
G56 Select coord system 3
G57 Select coord system 4
G58 Select coord system 5
G59 Select coord system 6
G59.1 Select coord system 7
G59.2 Select coord system 8
G59.3 Select coord system 9
G61 Set exact path mode
G61.1 Set exact stop mode Motion will stop between each G-code block
G64 P Q Continuous path mode Results in minimum execution time allowing minimal trajectory deformation
G65 P A B C … Macro call
G66 P A B C … Macro modal call
G67 Macro modal call cancel
G68 X Y Z R Coordinate System Rotation
G68.2 <X> <Y> <Z> I J K 3D plane rotation (arcs not supported) Rotate the reference plane in 3D so that G0,G1,G9 and cycles can be easily used on tilted planes. X ,Y,Z define the center of the rotation while I,J,K define the rotation around X, Y, Z. The order used to apply the rotation is always rotate around X, then Y, then Z. When G68.2 is active tool length compensation (G43, G43.1, …) can be enabled but tool radius compensation cannot be enabled.
G69 Cancel Coordinate System Rotation
G73 X Y Z R Q <L> High Speed Peck Drilling Cycle
Chip Break Drilling Cycle
G80 Cancel motion mode
G81 X Y Z R L Drilling Cycle
G82 X Y Z R L P Drilling Cycle, Dwell
G83 X Y Z R L Q Peck Drilling Cycle
G85 X Y Z R L Boring Cycle, Feed Out
G86 X Y Z R L P Boring Cycle, Spindle Stop, Rapid Move Out
G88 Boring Cycle, Spindle Stop, Manual Out
G89 Boring Cycle, Dwell, Feed Out
G90 Set absolute distance mode
G90.1 Set absolute arc distance mode Absolute distance mode for I, J & K offsets. When G90.1 is in effect I and J both must be specified with G2/3 for the XY plane or J and K for the XZ plane or it is an error
G91 Set incremental distance mode
G91.1 Set incremental arc distance mode Default arc mode
G92 axes Set origin offsets
G92.1 Reset origin offsets Reset parameters 5211 - 5219 to zero but G92 keeps its current state. Parameter 5210 remains 1 or 0 depending on its value before calling G92.1.
G92.2 Suspend origin offsets
G92.3 Resume origin offsets Set the G92 offsets to the values saved in parameters 5211 to 5219.
G93 Enable feed per inverse of time When this G code is processed the target feed is set to 60 (seconds) divided by the F<target feed> value.
G94 Enable feed per minute When this G code is processed the target feed is set to 0 and should be specified again using F<target feed>.
G98 Canned cycle return mode Initial Level Return In Canned Cycles set to initial Z
G99 Canned cycle return mode Initial Level Return In Canned Cycles set to R parameter
G100 P A B C … Internal PLC function Call
G101 P Set the axes to be interpolated Request the axes specified by the P parameter to be interpolated. The P parameter is a bitmask where bit 1 represents X axis, bit 2 Y axis, ….
G102 P Homing request Request the axes specified by the P parameter to be homed. The P parameter is a bitmask where bit 1 represents X axis, bit 2 Y axis, ….
G103 V Set traverse rate The maximum speed used for G0 motion. Units are mm/min. Zero means use the maximum value allowed by the axes involved in the movement.
G104 A D <J> Set interpolated motion dynamics Set the maximum acceleration and deceleration along the trajectory during interpolated motion. When A/D is set to 0 the maximum acceleration/deceleration allowed by the axes involved in the movement is used.
Units are mm/s^2 if G21 is active and inches/s^2 if G20 is active.
Example: G104 A100 D50 to set a maximum acceleration of 100 mm/s^2 and a maximum deceleration of 50 mm/s^2.
J is optional and can be used to set the jerk in % from 0.0 to 100.0. 0 Means accelerate with a slower ramp, 100% means accelerate immediately.
G200÷G499 A B C … User defined G codes User defined G codes require a user edited G-code file in macros folder with the G-code name (eg: g212.ngc).

Mcode Parameters Command Description
M0 Program Stop Current implementation place the CNC in PAUSE state.
M1 Program Optional Stop Current implementation place the CNC in PAUSE state if the optional stop input is on.
M2 Program End End a G-code program and reset the machine state: switch off I/O, mist, flood and spindle.
M3 Start spindle clock wise
M4 Start spindle counter clock wise
M5 Stop spindle turning
M6 Tool change See also User Tool Change Subprogram
M7 Mist On
M8 Flood On
M9 Mist and Flood Off
M17 Turn On Torch Height Control (THC)
M18 Turn Off Torch Height Control (THC)
M30 Pallet shuttle and program end If the correspondent settings is enabled the user G-code macro pallet_shuttle.ngc can be called.
M47 Restart program execution
M48 Enable the feed rate and spindle speed override controls
M49 Disable the feed rate and spindle speed override controls
M50 <P> Enable/Disable the feed rate override control.

P parameter is optional and if it is not specified P0 is considered.
Possible P values are:

  • 0 disable feed override
  • 1 enable feed override
  • 2 enable feed override custom 1
  • 3 enable feed override custom 2
M51 <P> Enable/Disable the spindle speed override control. Usage: M51 P1 (or M51) enable spindle speed override control and M51 P0 disable it. The P parameter is optional.
M60 Pallet shuttle If the correspondent settings is enabled the user G-code macro pallet_shuttle.ngc can be called.
M61 Q Set the current tool without performing a tool change. Could be called from user G-code defined tool change macro, see also User Tool Change Subprogram.
M62 P Turn out ON
M63 P Turn out OFF
M66 P L Q Wait input

Parameters:

  • P: the number of the user input signal to be waited
  • L:
    • 0: waits for the selected input to reach the LOW state
    • 1: waits for the selected input to reach the HIGH state
    • 2: waits for the selected input to perform a FALL event
    • 3: waits for the selected input to perform a RISE event
    • 4: return immediately and the input value is stored in #5720
    • 10 to 13: wait for the input to be LOW, HIGH, FALL or RISE and generate a CNC alarm if timeout elapses while waiting
  • Q: timeout in seconds (optional)

Notes:

  • If the correspondent compiler setting is enabled the input value is stored in parameter #5720 and can be used in the following control flow statements (IF, WHILE, …).
  • If the Q parameter is missing, the instruction waits until the condition is satisfied.
M67 P Read analog input Work the same way of M66 but is used to handle analog inputs
M68 P Q Set analog output Used instead of M62/M63 for analog outputs. Q argument is used to set the desired analog output value in percentage.
M98 P L Call Subroutine Note: a named external subroutine can be called
M99 Return from Subroutine
M102 End Program without reset End a program but does not perform an automatic reset switching off mist, flood, spindle status, …
M106 Execute PLC internal tool change procedure This M code is intended to be called by the user from the file named tool_change.ngc. This code inform the PLC to start the internal tool change procedure that can perform a few automatic actions not described by the procedure described using the G-code. See also User Tool Change Subprogram.
M107 Inform the PLC that the tool change procedure written in the User Tool Change Subprogram has started.
M108 Inform the PLC that the tool change procedure written in the User Tool Change Subprogram has ended.
M109 P Q D Show user message
M120 P Q D Show user media
M166 P Read digital input group The parameter P identifies the group. This M code updates the parameters #5740- #5759
M167 P Read input group The parameter P identifies the group. This M code updates the parameters #5740- #5759
M200÷M299 A B C … User defined M codes User defined M codes require a user edited G-code file with the macro name and .ngc extension to be place in the directory <%appdata%/RosettaCNC-1>/machines/<machine_name>/macros (eg: m210.ngc).

Simple G-code commands are used for setting the speed, feed, and tool parameters.

The F command sets the feed rate; the machine operates at the set feed rate when G1 is used, and subsequent G1 commands will execute at the set F value.

If the feed rate (F) is not set once before the first G1 call, either an error will occur or the machine will operate at its “default” feed rate.
An example of a valid F command: G1 F1500 X100 Y100

To see how RosettaCNC handled the feed rate when for single rotary axis moves or for mixed moves please check Feed Management

The S command sets the spindle speed, typically in revolutions per minute (RPM). An example of a valid S command: S10000

The T command is used to set the id of the tool to be loaded with the M6 command.
The typical syntax to load the tool with id 1 would be:
M6 T1

  • Setting the Tool Change Type option to Macro in the Board Settings the user can customize the tool change procedure.
    If the option is enabled the M06 command will look into the machine macros folder and execute the G-code file named tool_change.ngc.
    In this file the user can specify any supported G-code command to perform the tool change procedure as required by the specific machine.
    To see a reference implementation of the file tool_change.ngc please take a look to User Tool Change Subprogram.

The following syntaxes are supported:

  • (…) : simple comment between brackets
  • ; : simple comment till the end of the line started with a semi column

Block Delete, also called Optional Skip, determines what happens when a line of code has a forward slash mark (/).
In RosettaCNC integrated G-Code editor there is a dedicated icon to enable/disable this feature. When the feature is enabled and a line of G-Code begins with a forward slash the line is ignored and the execution skips to the next line of code.

  • Last modified: 2022/08/24 09:29
  • by cnc205