This is the manual of Studio 1.1.0, an earlier version. The manual of the latest version

G-code and M-code

The Twinwright controller (kernel) runs the G-code below. The codes follow RS274/NGC and LinuxCNC. A code the controller does not support answers error:20, and the line does nothing.

For the real-time commands (single bytes such as ?, ! and ~), see Protocol. For how the controller differs from other Grbl controllers, see The Twinwright controller.

G-code

Code	Meaning	Notes
`G0`, `G1`	Rapid move, linear feed
`G2`, `G3`	Arc clockwise, counter-clockwise (I J K or R), helix	The tool follows the true circle. An R-form arc with no chord in its plane answers `error:33`.
`G4 P`	Dwell, P seconds	The dwell lasts as long as programmed.
`G5`, `G5.1`	Cubic spline, quadratic spline	A `G5` without I and J continues in the direction the previous move ended.
`G7`, `G8`	Lathe diameter mode, radius mode	Lathe mode only (`$32=2`).
`G10 L2`, `G10 L20`	Set a work offset
`G10 L1`, `G10 L10`, `G10 L11`	Set the tool table	32 tools. The table is kept when the controller is off.
`G17`, `G18`, `G19`	Select the plane
`G20`, `G21`	Inch units, millimetre units
`G28`, `G30`	Go to a stored position through an intermediate point
`G28.1`, `G30.1`	Store the current position
`G33`, `G33.1`, `G76`	Spindle-synchronized motion, rigid tapping, threading cycle	These need a spindle encoder. The MC-1 has none, so they answer `error:20`.
`G38.2`–`G38.5`	Probe	The result is the point where the probe triggered, reported as `[PRB:]`. Set zero from that point, not from where the axes stopped.
`G40`	Cutter compensation off
`G41`, `G42`, `G41.1`, `G42.1`	Cutter radius compensation: D from the tool table, or `.1` with a diameter	G17 plane only. Entry and exit moves as in LinuxCNC. A move that would gouge is refused.
`G43 Hn`, `G43.2 Hn`	Tool length offset from the tool table, added offset
`G43.1`	Dynamic tool length offset
`G49`	Tool length offset off
`G50`, `G51`	Scaling off, on
`G52`	Local coordinate system	Shares its offset with `G92`, as in LinuxCNC.
`G53`	Machine coordinates for this line
`G54`–`G59`, `G59.1`–`G59.3`	Work coordinate systems	`$486` can lock `G59.1`–`G59.3`.
`G61`	Exact path
`G61.1`	Exact stop	The axes stop at the end of every programmed move.
`G64 P Q`	Path blending	Where it saves time, the corner between two straight moves becomes an arc within P of the corner. Q is accepted and not used.
`G65 P1`–`P6`	Built-in macros	Settings, tool offsets, parameters, machine state, probe choice, spindle wait. `P7` (Modbus messages) is not supported.
`G65 P100` and up, `G66`, `G66.1`, `G67`	File macros, modal macro calls	P must be an integer. No other command may share the line (`error:21`).
`G73`, `G81`, `G82`, `G83`	Drilling cycles, peck drilling	Each hole gets the pecks it needs.
`G84`, `G85`, `G86`, `G89`	Tapping and boring cycles
`G80`	Cycle off
`G90`, `G91`	Absolute distances, incremental distances
`G91.1`	Incremental arc centres
`G92`, `G92.1`, `G92.2`, `G92.3`	Coordinate offset: set, clear, suspend, restore
`G93`, `G94`, `G95`	Inverse time, units per minute, units per revolution	Arcs in inverse time take the programmed time.
`G96`, `G97`	Constant surface speed, constant spindle speed	Lathe mode only.
`G98`, `G99`	Cycle retract to the start height, to the R plane

These G-codes are not supported (error:20):

G5.2, G5.3 (NURBS);
G17.1–G19.1 (UVW planes);
G70–G72 (lathe cycles);
G90.1.

M-code

Code	Meaning	Notes
`M0`, `M1`	Program pause, optional pause	The `0x88` real-time command switches `M1` pauses on or off.
`M2`, `M30`	Program end
`M3`, `M4`, `M5`	Spindle clockwise, counter-clockwise, off
`M6`	Tool change	`$341` sets what M6 does. M6 and a motion in one line answer `error:40`.
`M7`, `M8`, `M9`	Coolant: mist, flood, off	On the MC-1, M8 runs the spindle's water cooling.
`M25`	Z up to the homed height	Centroid's code, written by some CAM post-processors.
`M48`, `M49`	Overrides on, off
`M50`–`M53`	Feed override, spindle override, adaptive feed, feed hold: on or off
`M56`	Parking on or off
`M60`	Pallet change pause
`M61`	Set the current tool without a change
`M62`–`M65`	Digital output on or off, with the next move or at once	On boards with auxiliary outputs.
`M66`	Wait for an input	The wait starts when the moves before it have ended.
`M70`–`M73`	Save and restore the modal state
`M98 P L`, `M99`	Call a subroutine, return	In programs run from the controller's file system. An `M98` sent line by line answers `error:39`. An `M99` in the main program ends it.

These M-codes are not supported (error:20):

M19 (spindle orientation);
M67, M68 (analog outputs; the MC-1 has none);
M100–M199 (user M-codes).

Words, syntax and parameters

Line structure

Comments ( … ) and ; are allowed.
(MSG,…) sends the text to the sender as a message.
(PRINT,…) sends a message with the values of the parameters it names.
(DEBUG,…) does the same while #5599 is on.
Block delete /, line numbers N and % lines (with or without a name) are allowed.
Case does not matter, and spaces inside words are ignored.

Parameters and expressions

Numbered parameters #1–#5000 belong to the program. They read 0 until the program sets them.
#5001 and up, and the named system parameters, can only be read.
Named parameters #<name>: reading a name that was never set answers error:39. EXISTS[#<name>] tells whether it was.
Expressions in [ ] use the operators and functions of LinuxCNC. Angles are in degrees.
A value that a line sets cannot be read in the same line.

O-words

Programs run from the controller's file system can use subroutines, if, elseif, else, while, do and repeat.
Subroutines and loops sent line by line are collected, then run when they are complete.
A subroutine can also be a file of its own: <name>.ngc, or <name>.macro.

Polar coordinates

@ is the radius and ^ the angle, in the XY plane around the work origin.

Errors in a line

Two codes of the same modal group in one line answer error:21.
Two commands that both use the axis words in one line answer error:24.
The full list of error codes is in Error codes.