G-codes: G00 G01 G02 G03 G04 G28 G38.2 G53 G90 G91 G92
M-codes: M00 M03 M04 M05 M62 M63 M66 M205 M410 M411 M666 M667

G-codes List

Code	Parameters	Description	Example
G00	X, Y, Z, A, B, C, F	Rapid positioning – moves the tool in a straight line to the specified coordinates. If no feedrate is provided, the machine uses maximum speed. Main parameters: • [X] – target X coordinate [mm] • [Y] – target Y coordinate [mm] • [Z] – target Z coordinate [mm] • [A] – target A coordinate [deg] • [B] – target B coordinate [deg] • ~~[C] – target C coordinate [mm]~~ Specify only the axes you want to move • [F] – feedrate [mm/min] If omitted, the machine moves at maximum speed Note: The C axis are not supported yet. Please refer to the product roadmap for details.	`G00 X10 Y20.52` Executes a rapid move from the current position to X10 Y20.52 at maximum speed. `G00 X30 Y40 F500` Executes a rapid move from the current position to X30 Y40 using a feedrate of 500 mm/min instead of the maximum speed.
G01	X, Y, Z, A, B, C, F	Linear interpolation – moves the tool in a straight line to the specified coordinates at the programmed feedrate. Main parameters: • [X] – target X coordinate [mm] • [Y] – target Y coordinate [mm] • [Z] – target Z coordinate [mm] • [A] – target A coordinate [deg] • [B] – target B coordinate [deg] • ~~[C] – target C coordinate [mm]~~ Specify only the axes you want to move • [F] – feedrate [mm/min] If omitted, uses the last feedrate specified for G01, G02, or G03 Note: The C axis is not supported yet. Please refer to the product roadmap for details.	`G01 X10 Y20.52 F500` Executes a linear interpolation from the current position to X10 Y20.52 at a feedrate of 500 mm/min. `G01 X30 Y40` Executes a linear interpolation from the current position to X30 Y40 using the last specified feedrate.
G02	X, Y, I, J, R, F	Circular interpolation, clockwise – moves the tool along a circular path in the XY plane to the specified end coordinates. Main parameters: • [X] – target X coordinate [mm] • [Y] – target Y coordinate [mm] Omitting X and Y executes a full circle at the current XY position when using the I/J center offset method. • [F] – feedrate [mm/min] If omitted, uses the last feedrate specified for G01, G02, or G03 The arc can be defined in two ways: (do not mix them in one line) 1. Center offset method: • [I] – X axis offset from the start point to the circle center [mm] • [J] – Y axis offset from the start point to the circle center [mm] At least one offset (I or J) must be specified when using this method. 2. Radius method: • [R] – circle radius [mm] The sign of R selects which arc is executed: R+ (positive value) – arc with sweep angle ≤ 180° R- (negative value) – arc with sweep angle > 180° Note: If R is provided, firmware uses the radius method and ignores I/J. The sign of R does not change the direction of motion. Direction is defined by the command – clockwise for G02.	`G02 X30 Y40 I10 J10 F100` CW arc to X30 Y40. Center is offset by I10 (X) and J10 (Y) from start point. Feedrate: 100 mm/min. `G02 X50 Y60 R15` CW arc to X50 Y60 with radius 15. R+ selects the shorter arc (≤ 180°). Uses last feedrate. `G02 X50 Y60 R-15` CW arc to X50 Y60 with radius 15. R- selects the longer arc (> 180°). Uses last feedrate. `G02 I10 J10` Full circle (360°) at current position with center offset I10 J10.
G03	X, Y, I, J, R, F	Circular interpolation, counterclockwise – moves the tool along a circular path in the XY plane to the specified end coordinates. Main parameters: • [X] – target X coordinate [mm] • [Y] – target Y coordinate [mm] Omitting X and Y executes a full circle at the current XY position when using the I/J center offset method. • [F] – feedrate [mm/min] If omitted, uses the last feedrate specified for G01, G02, or G03 The arc can be defined in two ways: (do not mix them in one line) 1. Center offset method: • [I] – X axis offset from the start point to the circle center [mm] • [J] – Y axis offset from the start point to the circle center [mm] At least one offset (I or J) must be specified when using this method. 2. Radius method: • [R] – circle radius [mm] The sign of R selects which arc is executed: R+ (positive value) – arc with sweep angle ≤ 180° R- (negative value) – arc with sweep angle > 180° Note: If R is provided, firmware uses the radius method and ignores I/J. The sign of R does not change the direction of motion. Direction is defined by the command – counterclockwise for G03.	`G03 X30 Y40 I10 J10 F100` CCW arc to X30 Y40. Center is offset by I10 (X) and J10 (Y) from start point. Feedrate: 100 mm/min. `G03 X50 Y60 R15` CCW arc to X50 Y60 with radius 15. R+ selects the shorter arc (≤ 180°). Uses last feedrate. `G03 X50 Y60 R-15` CCW arc to X50 Y60 with radius 15. R- selects the longer arc (> 180°). Uses last feedrate. `G03 I10 J10` Full circle (360°) at current position with center offset I10 J10.
G04	P, S	Dwell – pauses program execution for a specified period of time without moving the machine. Main parameters: • [P] – dwell time in milliseconds [ms] • [S] – dwell time in seconds [s] Only one parameter should be specified at a time. If both P and S are specified, the S parameter takes precedence. If no parameter is specified, or the value is 0 or negative, the command has no effect. Note: Before starting the dwell timer, firmware waits until all previously queued motion is complete. During dwell, the controller remains active.	`G04 P1000` Pauses execution for 1000 milliseconds (1 second). `G04 S2` Pauses execution for 2 seconds. `G04 P500 S1` Although P500 (500 ms) is specified, the S parameter takes precedence, resulting in a 1 second dwell. `G04` No parameters provided. The command is ignored and no dwell is performed. `G04 P0` Zero dwell time specified. The command has no effect.
G28	X, Y, Z, A, B, C, F, M, N, T, D, H	Homing and axis state control – controls homing, trust state and position reference of the specified axes. Main axis parameters: • [X] – target X axis • [Y] – target Y axis • [Z] – target Z axis • [A] – target A axis [deg] • [B] – target B axis [deg] • ~~[C] – target C axis~~ Operating modes: • [H] – return selected trusted axes to stored home position • [M] – manually set current position of selected axes to the provided coordinate values • [N] – manually set selected axes to machine zero / configured homing reference • [T] – mark selected axes as trusted and homed • [D] – mark selected axes as untrusted and unhomed If no mode parameter is given, automatic homing is performed. Automatic homing (default mode): Moves selected axes towards hardware endstops. Uses optional [F] feedrate or the configured homing feedrate if F is omitted or invalid. • Automatic homing order is Z, X, Y, A, B. Note: If multiple operating modes are provided in one command, firmware uses this priority: D > T > H > N > M > automatic homing. Note: The C axis is not supported yet. Please refer to the product roadmap for details.	`G28 X Y Z` Automatically homes X, Y and Z axes using hardware endstops. `G28 X0 Y0 M` Manually sets the current X and Y positions to the specified coordinates. `G28 X D` Marks the X axis as untrusted and unhomed. `G28 X T` Marks the X axis as trusted without performing any motion. `G28 X H` Moves the X axis to the stored home position (only if the axis is trusted). `G28 X N` Performs manual homing of the X axis using configured machine endstop limits. `G28 Z F100` Performs automatic homing of the Z axis using a custom feedrate.
G38.2	X, Y, Z, A, B, C, F	Probe towards material surface – moves the probe towards the specified target coordinates until material contact is detected. If the target Z position is reached without detecting material, an error is triggered. Main parameters: • [X] – target X coordinate [mm] • [Y] – target Y coordinate [mm] • [Z] – target Z coordinate [mm] • [A] – target A coordinate [deg] • [B] – target B coordinate [deg] • ~~[C] – target C coordinate~~ Specify only the axes you want to move. If no axis movement is requested, firmware only checks the current material detection input. • [F] – probing feedrate [mm/min] If omitted or invalid, the configured homing feedrate for the first moving axis is used.	`G38.2 Z-15 F500` Probes the Z axis down to -15 mm at 500 mm/min until material contact is detected. `G38.2 X50 Y50 Z-10` Moves towards the target position X50 Y50 Z-10. If material is detected before reaching Z-10, the probe stops immediately and the machine’s position is updated to X50 Y50, with Z set to the measured contact height.
G53	X, Y, Z, A, B, C, F	Move in the machine coordinate system – performs motion in the machine’s absolute coordinates, ignoring all work offsets. Main parameters: • [X] – target X absolute coordinate [mm] • [Y] – target Y absolute coordinate [mm] • [Z] – target Z absolute coordinate [mm] • [A] – target A absolute coordinate [deg] • [B] – target B absolute coordinate [deg] • ~~[C] – target C absolute coordinate~~ Specify only the axes you want to move • [F] – feedrate [mm/min] If omitted or invalid, the machine uses maximum feedrate	`G53 X0 Y0 Z0` Moves the machine to the absolute position X0 Y0 Z0 in the machine coordinate system at maximum speed (or specified F). Work offsets are ignored.
G90	–	Absolute positioning – all subsequent workspace moves are interpreted as absolute coordinates in the current work coordinate system. Note: Does not perform motion by itself; only changes how coordinates are interpreted. G53 always uses machine coordinates.	`G90` Sets the machine to absolute positioning mode. Future workspace movement commands use coordinates in the current work coordinate system. Example sequence: `G90 G0 X10 Y10` Moves the tool to absolute position X=10, Y=10. `G0 X20 Y5` Moves the tool to absolute position X=20, Y=5.
G91	–	Relative positioning – all subsequent workspace moves are interpreted as relative displacements from the current position. Note: Does not perform motion by itself; only changes how coordinates are interpreted. G53 always uses machine coordinates and is not affected by G91.	`G91` Sets the machine to relative positioning mode. Future workspace movement commands move the tool relative to its current position. Example sequence: `G91 G0 X10 Y10` Moves the tool +10 mm in X and +10 mm in Y relative to its current position. `G0 X-5 Y0` Moves the tool -5 mm in X, Y remains unchanged.
G92	X, Y, Z, A, B	Set logical current position – assigns the specified coordinates to the current position by shifting the workspace offset without moving the tool. Useful for resetting the origin or aligning workpieces. Main parameters: • [X] – X axis value to set [mm] • [Y] – Y axis value to set [mm] • [Z] – Z axis value to set [mm] • [A] – A axis value to set [deg] • [B] – B axis value to set [deg] • ~~[C] – C axis value to set~~ Note: The C axis is not supported yet. Please refer to the product roadmap for details.	`G92 X0 Y0 Z0` Sets the current machine position to X=0, Y=0, Z=0 without moving the tool. Future movement commands will interpret this as the new origin. `G92 X100` Sets the current X position to 100 mm, leaving other axes unchanged.
G92.38	–	Status: Not available yet. Planned for firmware FW 1.3. Set logical Z position from the last material detection input captured by G38. This command does not move the tool. Behavior: • If the last G38 detection used material input 1, Z is set using the configured material detect offset. • If the last G38 detection used material input 2, Z is set using the configured material detect 2 offset. • If no material detection input was captured by G38, the command is ignored. Note: Use G92.38 after a successful G38 probing move to apply the configured material detection offset to the logical Z position.	`G38.2 Z-15 F500 G92.38` Probes toward Z-15. If material is detected, G92.38 sets the logical Z position using the configured offset for the material detection input that was triggered.

M-codes List

Code	Parameters	Description	Example
M00	P, S	Program stop – pauses program execution until a continue signal is received. The signal can come from the user, an input pin, or an external module. Main parameters: • [P] – timeout in milliseconds • [S] – timeout in seconds Only one parameter should be specified at a time. If both P and S are specified, the S parameter takes precedence. If neither P nor S is specified, the timeout is 0 and firmware waits indefinitely for a continue signal. For ARC OK waiting, use M66 Q instead. M00 S timeout usage is legacy behavior and remains supported temporarily for backward compatibility.	`M00 S3` Stops program execution for up to 3 seconds or until a continue signal is received. If no signal is received within 3 seconds, firmware triggers a timeout fault and aborts the current file. `M00 P1000` Stops program execution for up to 1000 ms or until a continue signal is received. If no signal is received within 1000 ms, firmware triggers a timeout fault and aborts the current file. `M00` Stops program execution indefinitely until a continue signal is received.
M03	I	Turn ON the laser or plasma effector (activates main machine relay). Main parameters: • [I] – inline mode Enables effector in synchronization with move planner execution (inline mode). If omitted, the effector is turned on immediately after all previous motions are completed, without inline synchronization.	`M03` Turns on the effector by activating the main relay immediately after previous motions are done. `M03 I` Turns on the effector in inline mode, synchronized with planner execution.
M04	I	Turn ON the laser or plasma effector (activates main machine relay). Main parameters: • [I] – inline mode Enables effector in synchronization with move planner execution (inline mode). If omitted, the effector is turned on immediately after all previous motions are completed, without inline synchronization.	`M04` Turns on the effector by activating the main relay immediately after previous motions are done. `M04 I` Turns on the effector in inline mode, synchronized with planner execution.
M05	I	Turn OFF the laser or plasma effector (deactivates main machine relay). Main parameters: • [I] – inline mode Effector is disabled in synchronization with move planner execution (inline mode). If omitted, the effector is turned off immediately after all previous motions are completed, without inline synchronization.	`M05` Turns off the effector by deactivating the main relay immediately after previous motions are completed. `M05 I` Turns off the effector in inline mode, synchronized with planner execution.
M62	P, S, D, I	Turns ON a digital output (DO1-DO6) with optional power, idle value and inline synchronization. Main parameters: • [P] – output number (1-6) • [S] – output power in percent Optional; default 100%. Mainly affects continuous/PWM outputs. For binary outputs, any non-zero value turns the output ON. • [D] – idle value in percent Optional. Sets the output idle value before applying the command. Mainly affects continuous/PWM outputs. • [I] – inline mode Synchronizes output activation with motion execution. If omitted, firmware waits until all previous motions are completed, then turns the output on. Note: Continuous/PWM outputs are DO5 and DO6.	`M62 P3` Turns on digital output 3 after all previous motions are finished. `M62 P5 S75 I` Turns on continuous output 5 at 75% power, synchronized inline with motion planner execution. `M62 P6 D10` Sets the idle value of output 6 to 10%, then turns output 6 on at 100%.
M63	P, D, I	Sets a digital output (DO1-DO6) to its idle value with optional inline synchronization. Main parameters: • [P] – output number (1-6) • [D] – idle value in percent Optional. Sets the output idle value before applying the command. Mainly affects continuous/PWM outputs. • [I] – inline mode Synchronizes the output change with motion execution. If omitted, firmware waits until all previous motions are completed, then sets the output to its idle value. Note: For binary outputs this usually behaves as OFF. Continuous/PWM outputs are DO5 and DO6 and use their configured idle value.	`M63 P3` Sets digital output 3 to its idle value after all previous motions are finished. `M63 P5 I` Sets digital output 5 to its idle value in inline mode, synchronized with motion planner execution. `M63 P5 D10` Sets the idle value of output 5 to 10%, then applies that idle value to the output.
M66	Q	Status: Not available yet. Planned for firmware FW 1.3. Wait on input – pauses program execution until the ARC OK / continue signal is received or the timeout expires. Main parameters: • [Q] – timeout in seconds If Q is not specified, the timeout is 0 and firmware waits indefinitely for the input signal. M66 replaces the legacy M00 S timeout usage for ARC OK waiting. Legacy M00 S timeout usage is still supported temporarily for backward compatibility.	`M66 Q3` Waits for ARC OK / continue signal for up to 3 seconds. If no signal is received within 3 seconds, firmware triggers a timeout fault and aborts the current file. `M66` Waits indefinitely until ARC OK / continue signal is received.
M205	J, S, R	Set advanced machine settings – allows configuring internal motion parameters without moving the machine. Note: These settings are runtime settings. They are not stored permanently. After a power cycle or controller restart, default values are restored. Main parameters: • [J] – junction deviation in millimeters [mm] Affects how sharply the machine can change direction at corners. Use caution when increasing this value. • [S] – minimum steps per segment Valid range: 1-15. Values below 1 are ignored. Values above 15 are clamped to 15. • [R] – acceleration ramp type 0 = trapezoidal ramp, 1 = S-curve Bezier ramp. Note: Multiple parameters may be used in one command, for example M205 J0.05 S3 R1.	`M205 J0.05` Sets the junction deviation to 0.05 mm. `M205 S3` Sets the minimum steps per segment to 3. `M205 R1` Sets the acceleration ramp type to S-curve Bezier. `M205 J0.05 S3 R1` Updates junction deviation, minimum steps per segment and acceleration ramp type in one command.
M410	–	Emergency stop – immediately aborts all planned and active motion. The machine is stopped instantly, even in the middle of a move. Axis positions may become out of sync with the stepper position and should be re-homed before continuing. Note: This command is typically injected by the control system and should be used only in emergency situations.	`M410` Immediately stops all motion without deceleration (emergency stop).
M411	–	Controlled stop – aborts queued motions and performs a normal stop of the machine. Motion is stopped in a controlled manner. Unlike M410, this command uses a normal stop procedure and is safer for mechanics. Note: This command is typically injected by the control system.	`M411` Stops the machine using a controlled (non-emergency) stop.
M666	I	Disable Torch Height Controller (THC). Turns off automatic torch height regulation. Main parameters: • [I] – inline mode Disables THC in synchronization with motion planner execution. If omitted, firmware waits until all previous motions are completed, then disables THC.	`M666` Disables THC after the current motion queue is finished. `M666 I` Disables THC in inline mode, synchronized with motion execution.
M667	I, P, A	Enable Torch Height Controller (THC). Activates automatic torch height regulation during cutting operations. Main parameters: • [I] – inline mode Enables THC in synchronization with motion planner execution. If omitted, firmware waits until all previous motions are completed, then enables THC. • [P] – target voltage for THC Optional. P >= 0 sets manual target voltage. P-1 enables auto target voltage. Changing target voltage in inline mode is not supported and will be ignored. • [A] – antidive enable A > 0 enables antidive. A <= 0 disables antidive. Changing antidive in inline mode is not supported and will be ignored.	`M667` Enables THC with current settings after previous motions are completed. `M667 P120` Enables THC and sets the manual target voltage to 120 V. `M667 P-1` Enables THC and enables auto target voltage mode. `M667 A1` Enables THC and enables antidive. `M667 I` Enables THC in inline mode without changing target voltage or antidive settings.