Gcodes

NOTE: This page describes Gcode supported by g2core in firmware builds 100.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
  

This page and related pages describe basic Gcode commands for movement and parameters. Much of this is shamelessly cribbed from the LinuxCNC Gcode pages

Related Pages

• Mcodes
• G2, G3 Arc At Feed Rate
• G38.x Probes
• Coordinate Offsets and Coordinate Systems for G10, G53-G59, G92.x, JSON Offset commands

Gcode Summary

This table summarizes Gcode supported. 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
G5			Reserved for Spline Motion
G10 L2 G10 L20	axes, P	Set coord offsets
G17		Select XY arc plane
G18		Select XZ arc plane
G19		Select YZ arc plane
G20		Select inches mode	All Gcode from this point on will be interpreted in inches
G21		Select mm mode	All Gcode from this point on will be interpreted in millimeters
G28	axes	Goto G28 position	Optional axes specify an intermediate point
G28.1		Set G28 position	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	Goto G30 position	Optional axes specify an intermediate point
G30.1		Set G30 position	The current machine position is recorded (No parameters are provided)
G38.2	axes Fnnn	Probe	Probe toward, alarm if error
G38.3	axes Fnnn	Probe	Probe toward, do not alarm if error
G38.4	axes Fnnn	Probe	Probe away, alarm if error
G38.5	axes Fnnn	Probe	Probe away, do not alarm if error
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		Set exact path mode	Continuous motion between Gcode blocks - exact path will be traced
G61.1		Set exact stop mode	Motion will stop between each Gcode block
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	default arc 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		Set units-per-minutes feedrate mode / Cancel inverse feedrate mode
G95		Reserved for "Set units-per-revolution feedrate mode" (unimplemented)

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 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

G0 Straight Traverse (Rapid Move)

G0 'axes'
Straight traverse motion at maximum velocity

• All axis words are optional but must have a value if present. A traverse with no axes words will set motion mode to G0 but cause no movement
• G0 is optional if the current motion mode is G0
• It is expected that cutting will not take place when a G0 command is executing

The velocity will be the vector sum of the axes participating in the move, limited such that no participating axis will exceed it's maximum velocity, xVM in the axis settings. In some cases resultant toolhead velocity may exceed the velocities of the individual axes. For example, a move from (0,0) to (100,100) where xvm = 10,000 mm/min and yvm = 10,000 mm/min will execute at 14,143 mm/min as the resulting movement vector is sqrt(2)/2 x 10,000 mm/min.

the achievable velocity may also be limited by the jerk settings xJM for each participating axis. This occurs in the case where the move cannot achieve its maximum velocity due to jerk limitations in one or more axes. Jerk is also computed as a vector sum so that none of the participating axes will exceed their maximum jerk settings during the move.

G1 Straight Feed (Cutting Move)

G1 'axes' Fnnn causes straight feed motion at the requested feed rate or slower

• All axis words are optional but must have a value if present. A feed with no axes words will set motion mode to G1 but cause no movement
• G1 is optional if the current motion mode is G1
• F is optional if a feed rate is in effect. It is an error if no feed rate is in effect and none is specified.

Calculation of Feed Rate for Moves Including Rotary Axes

G2 adheres to the NIST Gcode definition for calculating feedrate for moves that include movement in A, B, C axes.

/*   2.1.2.5 Feed Rate
 *
 *  The rate at which the controlled point or the axes move is nominally a steady rate
 *  which may be set by the user. In the Interpreter, the interpretation of the feed
 *  rate is as follows unless inverse time feed rate mode is being used in the
 *  RS274/NGC view (see Section 3.5.19). The canonical machining functions view of feed
 *  rate, as described in Section 4.3.5.1, has conditions under which the set feed rate
 *  is applied differently, but none of these is used in the Interpreter.
 *
 *    A. For motion involving one or more of the X, Y, and Z axes (with or without
 *       simultaneous rotational axis motion), the feed rate means length units per
 *       minute along the programmed XYZ path, as if the rotational axes were not moving.
 *
 *    B. For motion of one rotational axis with X, Y, and Z axes not moving, the
 *       feed rate means degrees per minute rotation of the rotational axis.
 *
 *    C. For motion of two or three rotational axes with X, Y, and Z axes not moving,
 *       the rate is applied as follows. Let dA, dB, and dC be the angles in degrees
 *       through which the A, B, and C axes, respectively, must move.
 *       Let D = sqrt(dA^2 + dB^2 + dC^2). Conceptually, D is a measure of total
 *       angular motion, using the usual Euclidean metric. Let T be the amount of
 *       time required to move through D degrees at the current feed rate in degrees
 *       per minute. The rotational axes should be moved in coordinated linear motion
 *       so that the elapsed time from the start to the end of the motion is T plus
 *       any time required for acceleration or deceleration.
 */ 

Notes:

• When computing feed rate for a move, if one or more axis (linear or rotary) is not capable of meeting the acceleration/velocity to achieve the desired feed rate the move will be slowed down to accommodate the rate limiting axis, and hence a lower feed rate will be achieved.
• In case [A] above, if one or more rotary axes are involved in the move they will complete their motion(s) in the same time that the linear axes are moving. It is possible that the rotary axis (axes) may rate limit the move as described above.
• For g2core builds that support UVW axes g2core extends the NIST definition to include all linear axes (XYZ & UVW) when calculating feed rates.

G2, G3 Arc At Feed Rate

See G2, G3 Arc At Feed Rate

G4 Dwell

G4 Pnnn causes motion to stop and resume nnnn seconds later

• The P number is a required floating point number; fractions of a second may be used
• G4 affects spindle, coolant and I/O as programmed (details of this are currently incomplete and not listed)

G5 Reserved for Spline Motion

Currently spline motion is not supported.

G10 Offsets

See G10 coordinate offsets

G17, G18, G19 Select Arc Plane

G17 select XY arc plane G18 select XZ arc plane G19 select YZ arc plane

G20, G21 Select Units Mode

G20 selects inches mode
G21 selects millimeter mode

G28, G30 Go To Predefined Position

G28.1 save location of current point in absolute coordinates
G28 return to point saved in g28.1
G28 axes return to point saved in g28.1 through intermediate point in axes

G30.1 save location of current point in absolute coordinates
G30 return to point saved in g30.1
G30 axes return to point saved in g30.1 through intermediate point in axes

• G28 (and G30) will move the machine to absolute coordinates set in G28.1 (G30.1) at traverse rate (G0)
• If G28.1 or G30.1 is not set the return point is (0,0,0,0,0,0)
• If 'axes' are provided the move will proceed through the intermediate point specified
• Axes that are not specified in the G28 or G30 command are not included in the intermediate move
• Movement will occur in the machine coordinate system (absolute coordinates, G53), and is not affected by work coordinate systems (G54-G59), temporary offsets (G92), or tool length offsets. However, position reporting {pos:n} will be provided using all offsets in effect at the time of the G28/G30 command.

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.

G38.x Probes

See G38.x Probes

G53, G54, G55, G56, G57, G58, G59 Coordinate systems

See Coordinate Systems.

G61, G64 Path Control Modes

G61 set exact path mode
G61.1 set exact stop mode
G64 set continuous mode (behaves like exact path mode)

G2core supports exact path mode (G61) and exact stop 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 the jerk limits of the participating axes.

G80 Cancel Motion Mode

G80 cancel motion mode

G80 cancels the current motion mode. Send G80 to make sure no movement will occur. Motion modes are the NIST Gcode modal group 1, which includes: G0, G1, G2, G3, G38.2, G80, G81, G82, G83, G84, G85, G86, G87, G88, G89

G90, G91 Set Distance Mode

G90 set absolute distance mode (default)
G91 set incremental distance mode
G90.1 set absolute arc distance mode
G91.1 set incremental arc distance mode (default)

In absolute distance mode, axis positions are provided as absolute coordinates in the currently active coordinate system. In incremental distance mode, axis positions represent incremental movement from the current point.

G92, G92.x

See Coordinate Systems.

G93, G94, G95 Feed Rate Mode

G93 set inverse-time feedrate mode
G94 set units-per-minutes feedrate mode
G95 reserved for set units-per-revolution feedrate mode (unimplemented)