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.

1.4 G-Code Comments

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.