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
• G38.x Probes
• Coordinate Offsets 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](#g0-straight-traverse-rapid-move) | _axes_ | Straight traverse | Traverse at maximum velocity
[G1](#g1-straight-feed-cutting-move) | _axes_ F | Straight feed | Move at feed rate F
[G2](#g2-g3-arc-at-feed-rate) | _axes_ F P  IJK or R | Clockwise arc feed | Arc at feed rate F
[G3](#g2-g3-arc-at-feed-rate) | _axes_ F P  IJK or R | Counterclockwise arc feed | Arc at feed rate F
[G4](#g4-dwell) | P | Dwell | Pause for P seconds
[G10 L2](Gcode-Coordinate-Offsets#g10-ln-set-parameters) [G10 L20](Gcode-Coordinate-Offsets#g10-ln-set-parameters)  | _axes_, P | Set coord offsets
[G17](Gcode-Circular-Arcs#g17-g18-g19-select-arc-plane) | | Select XY arc plane |
[G18](Gcode-Circular-Arcs#g17-g18-g19-select-arc-plane) | | Select XZ arc plane |
[G19](Gcode-Circular-Arcs#g17-g18-g19-select-arc-plane) | | Select YZ arc plane |
[G20](#g20-g21-select-units-mode) | | Select inches mode | All Gcode from this point on will be interpreted in inches
[G21](#g20-g21-select-units-mode) | | Select mm mode | All Gcode from this point on will be interpreted in millimeters
[G28](#g28-g30-go-to-predefined-position) | _axes_ | Goto G28 position | Optional axes specify an intermediate point
[G28.1](#g28-g30-go-to-predefined-position) | | Set G28 position | The current machine position is recorded (No parameters are provided)
[G28.2](https://github.com/synthetos/TinyG/wiki/Homing-and-Limits-Description-and-Operation#g282---homing-sequence-homing-cycle) | _axes_ | Homing Sequence | Homes all axes present in command. At least one axis must be specified
[G28.3](https://github.com/synthetos/TinyG/wiki/Homing-and-Limits-Description-and-Operation#g283---set-absolute-position) | _axes_ | Set Absolute Position | Set axis to zero or other value. Use to zero axes that cannot otherwise be homed
[G30](#g28-g30-go-to-predefined-position) | _axes_ | Goto G30 position | Optional axes specify an intermediate point
[G30.1](#g28-g30-go-to-predefined-position) | | Set G30 position | The current machine position is recorded (No parameters are provided)
[G38.2](Gcode-Probes#g38x-probe) | _axes_ | Probe | Probe toward, do not report error 
[G38.3](Gcode-Probes#g38x-probe) | _axes_ | Probe | Probe toward, report if error 
[G38.4](Gcode-Probes#g38x-probe) | _axes_ | Probe | Probe away, do not report error 
[G38.5](Gcode-Probes#g38x-probe) | _axes_ | Probe | Probe away, report if error 
[G53](Gcode-Coordinate-Offsets) | | Select absolute coordinates | Non-Modal: Applies only to current block
[G54](Gcode-Coordinate-Offsets) | | Select coord system 1 | G54 is typically used as the "normal" coordinate system and reflects the machine position
[G55](Gcode-Coordinate-Offsets) | | Select coord system 2 |
[G56](Gcode-Coordinate-Offsets) | | Select coord system 3 |
[G57](Gcode-Coordinate-Offsets) | | Select coord system 4 |
[G58](Gcode-Coordinate-Offsets) | | Select coord system 5 |
[G59](Gcode-Coordinate-Offsets) | | Select coord system 6 |
[G61](#g61-g64-path-control-modes) | | Exact stop mode | Motion will stop between each Gcode block
[G61.1](#g61-g64-path-control-modes) | | Exact path mode | Continuous motion between Gcode blocks - exact path will be traced
[G64](#g61-g64-path-control-modes) | | Continuous path mode | Same as exact path mode 
[G80](#g80-cancel-motion-mode) | | Cancel motion mode |
[G90](#g90-g91-set-distance-mode) | | Set absolute distance mode |
[G90.1](Gcode-Circular-Arcs#g901-g911-arc-distance-mode) | | Set absolute arc distance mode |
[G91](#g90-g91-set-distance-mode) | | Set incremental distance mode |
[G91.1](Gcode-Circular-Arcs#g901-g911-arc-distance-mode) | | Set incremental arc distance mode | default arc mode
[G92](Gcode-Coordinate-Offsets) | _axes_ | Set origin offsets |
[G92.1](Gcode-Coordinate-Offsets) | | Reset origin offsets |
[G92.2](Gcode-Coordinate-Offsets) | | Suspend origin offsets |
[G92.3](Gcode-Coordinate-Offsets) | | Resume origin offsets |
[G93](#g93-g94-g95-feed-rate-mode) | | Set inverse feedrate mode |
[G94](#g93-g94-g95-feed-rate-mode) | | Cancel inverse feedrate mode |


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.
[()](#gcode-comments) | [comment](#gcode-comments) | [gcode comment](#gcode-comments) | Gcode comments are supported. They are stripped and ignored, except for messages (below)
[;](#gcode-comments) | 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.

##G2, G3 Arc At Feed Rate G2 or G3 'axes' 'offsets' Pn Fnnn center format arc
G2 or G3 'offsets' Pn Fnnn center format full circle arc
G2 or G3 'axes' Rnnn Pn Fnnn radius format arc
G2 or G3 Rnnn Pn Fnnn radius format full circle arc

• 'axes' are any of XYXABC
• 'offsets' are any of IJK

Note: Much of this specification has been copied from Linux CNC Gcode, G2-G3, but they are not identical as some differences exist.

A circular or helical arc is specified using either G2 (clockwise arc) or G3 (counterclockwise arc) at the current feed rate F. The direction (CW, CCW) is as viewed from the positive end of the axis about which the circular motion occurs.

• The axis of the circle or helix must be parallel to the X, Y, or Z axis of the machine coordinate system. The axis (or, equivalently, the plane perpendicular to the axis) is selected with G17 (Z-axis, XY-plane), G18 (Y-axis, XZ-plane), or G19 (X-axis, YZ-plane). If the arc is circular, it lies in a plane parallel to the selected plane.

• To produce a helix include the axis word perpendicular to the arc plane: for example, if in the G17 plane, include a Z word. This will cause the Z axis to move to the programmed value during the circular XY motion.

• To program an arc that gives more than one full turn use the P word specifying the number of full turns plus the programmed arc. The P word must be an integer. If P is unspecified, the behavior is as if P1 was given: that is, only one full or partial turn will result. For example, if a 180 degree arc is programmed with a P2, the resulting motion will be 1 1/2 rotations. For each P increment above 1 an extra full circle is added to the programmed arc. Multi-turn helical arcs are supported and give motion useful for milling holes or threads.

• If a line of code makes an arc and includes rotary axis motion the rotary axes turn at a constant rate so that the rotary motion starts and finishes when the XYZ motion starts and finishes. Lines of this sort are hardly ever programmed.

• The arc center is absolute or relative as set by G90.1 or G91.1 respectively.

• Two formats are allowed for specifying an arc: Center Format and Radius Format.

It is an error if:

• No feed rate has been set
• The P word is not an integer

###Center Format Arcs Center format arcs are more accurate than radius format arcs and are the preferred format to use.

• The end point of the arc ('axes') along with the offset to the center of the arc from the current location ('offsets') are used to program arcs that are less than a full circle

• It is OK if the end point of the arc is the same as the current location, but these arcs will have no movement. They are not treated as a full circle arc. For full circle arcs the endpoints must be omitted.

• The offset to the center of the arc from the current location and optionally the number of turns are used to program full circles. For full circle arcs no 'axes' words should be provided.

• When programming arcs an error due to rounding can result from using a precision of less than 4 decimal places (0.0000) for inch and less than 3 decimal places (0.000) for millimeters.

####Incremental Arc Distance Mode Incremental Arc Distance Mode is the default mode, and may be set by G91.1. The following applies:

• Arc center offsets are a relative distance from the start location of the arc
• One or more axis words and one or more offsets must be programmed for an arc that is less than 360 degrees
• No axis words and one or more offsets must be programmed for full circles. The P word defaults to 1 and is optional

####Absolute Arc Distance Mode Absolute Arc Distance Mode may be set by G90.1. The following applies:

• Arc center offsets are the absolute distance from the current 0 position of the axis
• One or more axis words and both offsets must be programmed for arcs less than 360 degrees
• No axis words and both offsets must be programmed for full circles. The P word defaults to 1 and is optional

####XY-Plane Arcs (G17) G2 or G3 Xnnn Ynnn Znnn Innn Jnnn Pn

• X, Y - Endpoint, or omitted for full-circle arc
• Z - helix travel (optional)
• I - X offset
• J - Y offset
• K - Z offset MUST NOT BE PRESENT
• P - number of turns (optional, must be integer)

####XZ-Plane Arcs (G18) G2 or G3 Xnnn Znnn Ynnn Innn Knnn Pn

• X, Z - Endpoint, or omitted for full-circle arc
• Y - helix travel (optional)
• I - X offset
• J - Y offset MUST NOT BE PRESENT
• K - Z offset
• P - number of turns (optional, must be integer)

####YZ-Plane Arcs (G19) G2 or G3 Ynnn Znnn Xnnn Jnnn Knnn Pn

• Y, Z - Endpoint, or omitted for full-circle arc
• X - helix travel (optional)
• I - X offset MUST NOT BE PRESENT
• J - Y offset
• K - Z offset
• P - number of turns (optional, must be integer)

For any of the the G17, G18, G19 arcs, it is an error if:

• No feed rate is set with the F word
• No offsets are programmed
• An illegal offset is present
• When the arc is projected on the selected plane, the distance from the current point to the center differs from the distance from the end point to the center by more than (.05 inch/.5 mm) OR ((.0005 inch/.005mm) AND .1% of radius).

###Radius Format Arcs G2 or G3 Xnnn Ynnn Znnn Rnnn Fnnn
G2 or G3 Rnnn Pn Fnnn

In the radius format the coordinates of the end point of the arc in the selected plane are specified along with the radius of the arc.

• The axis words are optional except at least one of the two words for the axes in the selected plane must be used
• The R number is the radius
• A positive radius indicates that the arc turns through less than 180 degrees, while a negative radius indicates a turn of more than 180 degrees
• If the arc is helical, the value of the end point of the arc on the coordinate axis parallel to the axis of the helix is also specified.

It is an error if:

• Both of the axis words for the axes of the selected plane are omitted
• The end point of the arc is the same as the current point

It is not good practice to program radius format arcs that are nearly full circles or nearly semicircles because a small change in the location of the end point will produce a much larger change in the location of the center of the circle (and, hence, the middle of the arc). The magnification effect is large enough that rounding error in a number can produce out-of-tolerance cuts. For instance, a 1% displacement of the endpoint of a 180 degree arc produced a 7% displacement of the point 90 degrees along the arc. Nearly full circles are even worse. Other size arcs (in the range tiny to 165 degrees or 195 to 345 degrees) are OK.

##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.

##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 'axes' return to point saved in g28.1 - through intermediate point if 'axes' present
G28.1 save location of current point in absolute coordinates
G30 'axes' return to point saved in g30.1 - through intermediate point if 'axes' present
G30.1 save location of current point in absolute coordinates

• G28 (and G30) will move the machine to the absolute coordinates set in G28.1 (G30.1)
• Movement will occur at the traverse rate (G0 rate)
• If 'axes' are provided the move will proceed through the intermediate point specified
• Axes that are not specified are ignored (not moved)
• Movement will always 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

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, G64 Path Control Modes G61 set exact stop mode
G61.1 set path stop mode
G64 set continuous mode (behaves like exact path mode

G2core 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 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 abopsulte coordinates in the currently active coordinate system. In incremental distance mode axis positions represent incremental movement from the current point.

##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)