Gcode Support

NOTE: This page describes Gcode supported by TinyG in firmware versions 0.95 and later

See also:

• Feedhold and Cycle Start (Pause and Resume)
• Homing and Limits

TinyG implements the NIST RS274v3/ngc dialect of Gcode. We try to adhere as closely as possible to the NIST Gcode and LinuxCNC Gcode specifications:

• 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. At least one axis must be present
G1	axes, F	Straight feed	Feed at feed rate F. At least one axis must be present
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
G17		Select XY plane	G17, G18 and G19 set the plan 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)
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 path mode	Continuous motion between Gcode blocks - exact path will be traced - stops only if it must
G61.1		Exact stop mode	Motion will stop between each Gcode block
G64		Continuous path mode	Sacrifice path following accuracy in order to keep the feed rate up
G80		Cancel motion mode
G90		Set absolute mode
G91		Set incremental 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
M114		Get current position	Report the current coordinates
M115		Get Firmware	Report the current firmware, version and capabilities
M201.3	axes	Set axes jerk	Set transient axis jerk rate
M400		Finish moves	Wait for current moves to finish

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 Set Parameters (Offsets)

Currently the only G10 command supported is G10 L2, which is used to set coordinate offsets. Use Pn to select coordinate system 1-6 (G54 - G59, respectively), and one or more axis value to set the offset for that axis. The format is:

G10 L2 P1 X0 Y0 Z0 A0 B0 C0  - set G54 offsets to zero, making G54 act as persistent absolute coordinates

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 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 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)

M114 Get current Position

Reports the current target position.

Example:

M114

X:100.0000 Y:0.0000 Z:0.0000 A:0.0000 B:0.0000 C:0.0000

M115 Get Firmware, Version and Capabilities

Reports the firmware, version and capabilities as many other controllers do. This allows Gcode generating software connected to an initially unknown controller to automatically detect it and adapt itself accordingly. Gcode generating software can then provide a "Plug-and-Play" experience to the user.

Example:

M115

FIRMWARE_NAME:TinyG, FIRMWARE_URL:https%3A//github.com/synthetos/TinyG, FIRMWARE_VERSION:0.97, FIRMWARE_BUILD:440.21, HARDWARE_PLATFORM:1.00, HARDWARE_VERSION:8.00

M201.3 Set jerk

Sets the jerk of one or more axes transiently. Axis jerk rates are given in units per second³ in order to remain compatible to analogous M201 commands on other controllers. The jerk rates are internally converted to TinyG's km per minute³ rate. Note, $xjm, $yjm etc. remain unaffected by the transient setting.

Example:

M201.3 X90000 Z10000

Watch a video of how this is useful for the OpenPnP software:

https://youtu.be/6SBDApObbz0

M400 Wait for current moves to finish

Some Gcode generating application (e.g. OpenPnP) need to interact in real-time with the machine. One example: A camera is moved to a location, then Computer Vision is used. Obviously, the application needs to know when the camera has arrived, before it can take a picture.

M400 blocks all further command processing, until the move buffers have drained. The acknowledgement "tinyg ok>" is only reported once this has happened. The application can therefore synchronize itself efficiently with TinyG.

Example:

G1 X100
M400   ; wait for the move to complete
M114   ; only now report the position

Gcode Comments

• Comments start with a '(' char or alternately a semicolon ';'
• Comments always terminate the block - i.e. leading or embedded comments are not supported

Valid comment cases       Notes:
G0X10                      - command only - no comment
G0X10 (comment text)       - command with comment
G0X10 (comment text        - it's OK to drop the trailing paren
G0X10 ;comment text        - comment delimited by semicolon (firmware build 378.05 and later)
(comment text)             - there is no command on this line

Invalid comment cases     Notes:
G0X10 comment text         - comment with no separator
N10 (comment) G0X10        - embedded comment. G0X10 will be ignored
(comment) G0X10            - leading comment. G0X10 will be ignored
G0X10 #comment             - invalid comment separator