Gcode Support

NOTE: This page describes Gcode supported by G2 in firmware builds 083.xx and later

G2 implements the NIST RS274v3/ngc dialect of Gcode informed by the LinuxCNC Gcode specification:

• Kramer's NIST RS274NGCv3 Gcode Specification
• LinuxCNC Gcode Specification
  

Cheat Sheet

This table summarizes Gcode supported. axes means one or more of X,Y,Z,A,B,C.

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, I,J,K or R	Clockwise arc feed	Arc at feed rate F. Offset mode IJK or radius mode R
G3	axes, F, I,J,K or R	Counter clockwise arc feed	Arc at feed rate F. Offset mode IJK or radius mode R
G4	P	Dwell	Pause for P seconds
G10 L2	axes, P	Set offset parameters	P selects coordinate system 1-6
G10 L20	axes, P	Set offset parameters	P selects coordinate system 1-6
G17		Select XY plane	G17, G18 and G19 set the plane in which the G2/G3 arcs are drawn
G18		Select XZ plane
G19		Select YZ plane
G20		Select inches units mode	All Gcode from this point on will be interpreted in inches
G21		Select mm units mode	All Gcode from this point on will be interpreted in millimeters
G28	axes	Go to G28.1 position	Optional axes specify an intermediate point
G28.1		Set position for G28	The current machine position is recorded (No parameters are provided)
G28.2	axes	Homing Sequence	Homes all axes present in command. At least one axis must be specified
G28.3	axes	Set Absolute Position	Set axis to zero or other value. Use to zero axes that cannot otherwise be homed
G30	axes	Go to G30.1 position	Optional axes specify an intermediate point
G30.1		Set position for G30	The current machine position is recorded (No parameters are provided)
G38.2	axes	Probe toward, do not report error	Supported in Build 082.xx
G38.3	axes	Probe toward, report if error	Supported in Build 100.xx
G38.4	axes	Probe away, do not report error	Supported in Build 100.xx
G38.5	axes	Probe away, report if error	Supported in Build 100.xx
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
G61		Exact stop mode	Motion will stop between each Gcode block
G61.1		Exact path mode	Continuous motion between Gcode blocks - exact path will be traced
G64		Continuous path mode	Same as exact path mode
G80		Cancel motion mode
G90		Set absolute distance mode
G90.1		Set absolute arc distance mode
G91		Set incremental distance mode
G91.1		Set incremental arc distance mode
G92	axes	Set origin offsets
G92.1		Reset origin offsets
G92.2		Suspend origin offsets
G92.3		Resume origin offsets
G93		Set inverse feedrate mode
G94		Cancel inverse feedrate mode

Mcode	Parameter	Command	Description
M0		Program stop
M1		Program stop	Optional program stop switch is not implemented so M1 is equivalent to M0
M2		Program end
M30		Program end
M60		Program stop
M3	S	Spindle on - CW	S is speed in RPM
M4	S	Spindle on - CCW	S is speed in RPM
M5		Spindle off
M6		Change tool	No operation at this time
M7		Mist coolant on	Note that mist and flood share the same Coolant ON/OFF pin
M8		Flood coolant on	Note that mist and flood share the same Coolant ON/OFF pin
M9		All coolant off	Note that mist and flood share the same Coolant ON/OFF pin

Other	Parameter	Command	Description
N	line number	label gcode block	Line numbers are allowed, handled, and may be reported back in status reports. Don't underestimate how useful this is for debugging Gcode files.
()	comment	gcode comment	Gcode comments are supported. They are stripped and ignored, except for messages (below)
;	comment	alternate comment	A semicolon is an alternate way to delimit a comment. This is not Gcode "standard", but is used by Mach and some Reprap codes. (available as of build 378.05)
(msg....)	message	gcode message	Gcode messages are comments that begin with the characters msg (case insensitive). These will be echoed to the operator

Gcode Reference

Some of the more complicated commands are described here. Much of this is shamelessly cribbed from the LinuxCNC Gcode pages

G10 L2 Set Parameters (Offsets)

The G10 L2 command is used to set coordinate offsets. Use Pn to select coordinate system 1-6 (G54 - G59, respectively), and one or more axis values to set the offset for that axis. The axis value is the offset you want for that axis, relative the zero set during homing. For example, if you wanted the X origin of coordinate system 1 (G54) to be 100 mm to the right of zero you would enter G10 L2 X100.

G10 L20 Set Parameters (Offsets)

The G10 L20 command is also used to set coordinate offsets. Use Pn to select coordinate system 1-6 (G54 - G59, respectively), and one or more axis values to set the offset for that axis. The axis value is the value you wish the current point to be. For example, if you wanted the current X location to be X0 in coordinate system 1 (G54) you would enter G10 L20 X0.

G28, G28.1, G30, G30.1 Go To Predefined Position

G28 (and G30) will move the machine to the absolute coordinates set in G28.1 (G30.1), optionally through an intermediate point. Movement will occur at the traverse rate (G0 rate). Axes that are not specified are ignored (not moved). The axis value is the intermediate point for that axis.

Format is:

G28 X0 Y0 Z0 A0 B0 C0

Gcode	Parameters	Command	Description
G28	axes	Go to G28.1 position	Goes through intermediate point if axes are present
G28.1		Set position for G28	Axes are not used and are ignored if present
G30	axes	Go to G30.1 position	Goes through intermediate point if axes are present
G30.1		Set position for G30	Axes are not used and are ignored if present

Example of use:

• Go to an arbitrary position, e.g. G0 x100 y100
• Send G28.1 - This will "remember" the absolute position. This position remains constant regardless of what coordinate system is in effect.
• Then go to a different place, e.g. G0 x50 y50
• Send G28 - The machine will return to x100 y100

Example:

• Go back to X0Y0
• Send G91 G28 Z10 - this will move to x100 y100. The tool will initially lift z by 10 mm (or inches); G91 is used to set relative mode for this command.

G61, G61.1, G64 Path Control Modes

TinyG supports exact stop mode (G61) and exact path mode (G61.1). G64 is recognized, but is treated as exact path mode. In exact stop mode motion will stop between each Gcode block. In exact path mode the exact path is followed (i.e. corners are not rounded). The velocity at the points joining 2 blocks is controlled to keep the change in direction between the blocks within centripetal acceleration limit set by $JA. Please see here for an explanation.

M2, M30 Program End

program END (M2, M30) performs the following actions:

• Axis offsets are set to G92.1 CANCEL offsets
• Set default coordinate system (uses $gco)
• Selected plane is set to default plane ($gpl)
• Distance mode is set to MODE_ABSOLUTE (like G90)
• Feed rate mode is set to UNITS_PER_MINUTE (like G94)
• The spindle is stopped (like M5)
• Motion mode is canceled like G80 (not set to G1)
• Coolant is turned off (like M9)
• Default INCHES or MM units mode is restored ($gun)

Gcode Comments

Gcode comments possess a number of features that extend their capabilities beyond classic Gcode. This is to support active comments and other developments. Please see Gcode Comments