GCodes

The below table shows the supported GCodes

Gcode	function	example
G0	Move to the given coordinates. It is used to go to a new area without cutting, it is also called a “rapid” move. Note that the F parameter can be used here and is remembered by subsequent commands	G0 X10 Y5 F100
G1	Move to the given coordinates, see above for the difference with G0. Takes the same F parameter as G0	G1 X20 Y2.3 F200
G2	Clockwise circular motion : go to point with coordinates XYZ while rotating around point with relative coordinates IJ	G2 X10 J5
G3	Counter-clockwise motion : see above	G3 Y5 X10 I2
G4	Dwell P<seconds>	G4 P1
G10	Set workspace coordinates http://linuxcnc.org/docs/html/gcode/coordinates.html and http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g10-l2	G10 L2 P1 X0
G17	Select XYZ plane (command is modal)	G17
G18	Select XZY plane (command is modal)	G18
G19	Select YZX plane (command is modal)	G19
G20	Inch mode : passed coordinates will be considered as Inches, so internally translated to millimeters	G20
G21	Millimeter mode ( default ) : passed coordinates will be considered as millimeters	G21
G23	select file	not used
G24	start print	not used
G25	pause print	not used
G26	reset print	not used
G27	report print progress
G28	G28 means goto clearance position on the Carvera	G28
G29	wait for empty queue. investigate more
G31	same as G32, ignore
G32	G32 probes the grid and turns the compensation on, this will remain in effect until reset or M370, X and Y are the start position, A and B are the width and length, I and J are the grid size, H is the height.	G32 R1 X0 Y0 A10 B10 H2
G38	Standard probe commands implemented as documented here	G38.2 Z-10
G38.2	probe toward workpiece, stop on contact, signal error if failure
G38.3	probe toward workpiece, stop on contact
G38.4	probe away from workpiece, stop on loss of contact, signal error if failure
G38.5	probe away from workpiece, stop on loss of contact,
G38.6	calibrate z, function unclear further testing required. Hard Disabled in Firmware
G53	Must be on a line by itself OR the first G code on a line, the directly following G0/G1 will be executed in MCS coordinates	G53 G0 X0 Y0
G54	Use workspace coordinates http://linuxcnc.org/docs/html/gcode/coordinates.html and http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g54-g59.3	G54
G55-59	same as G54
G90	Absolute mode ( default ) (command is modal)	G90
G91	Relative mode (command is modal)	G91
G92	Set global workspace coordinate system to specified coordinates http://linuxcnc.org/docs/html/gcode/g-code.html#gcode:g92	G92 X0 Y0 Z0
G92.1	Clear the G92 offsets	G92.1
G92.4	Manually set homing (MCS) for XYZ	G92.4 X0 Y0 Z0
G92.4 A0 S0	shrink a axis back to zero-360, useful for continous rotation machining