G-Code Reference Guide

G00 — Rapid Positioning

Moves the tool to the specified position at the machine's maximum traverse rate. Used for non-cutting moves — repositioning between cuts, moving to the start position, or retracting the tool. The path is not guaranteed to be a straight line on all machines.

Rapid move to X=1.0, Y=2.0, Z=0.5

G01 — Linear Interpolation

Moves the tool in a straight line to the specified position at the programmed feed rate (F). This is the primary cutting command — use it whenever you need the tool to follow a controlled, straight-line path through material.

Linear move to X=2.0, Y=3.0 at feed rate 100. Second line adds a Z plunge.

G02 — Circular Interpolation (Clockwise)

Moves the tool in a clockwise arc. The arc center is defined relative to the start point using I/J/K offsets, or by specifying the radius with R. I is the X offset to center, J is the Y offset, and K is the Z offset.

Both produce a clockwise arc with radius 1.0 ending at X=2.0, Y=0.0.

G03 — Circular Interpolation (Counter-Clockwise)

Same as G02 but the arc goes counter-clockwise. Uses the same I/J/K or R syntax.

G04 — Dwell

Pauses program execution for the specified duration. The parameter P specifies the dwell time. On most controllers, P is in seconds; on some older machines, it may be in milliseconds — check your controller's documentation.

Pauses for 1.5 seconds.

G10 — Set Coordinate Data

Sets work coordinate offsets or tool data programmatically without manually editing the controller's offset table. Commonly used to set work offsets (G54–G59) from within a program.

L2 = work coordinate offset, P1 = G54 (P2 = G55, etc.)

G17 / G18 / G19 — Plane Selection

Selects the active plane for arc commands (G02/G03). The plane determines which two axes define the arc and which axis is the helical axis.

G17 (XY plane) is the default on most machines and the most commonly used.

G20 / G21 — Units Selection

Sets the unit of measurement for all subsequent commands.

Always set units at the start of your program. Mismatched units are one of the most common causes of CNC errors.

G28 — Return to Home Position

Returns the machine to its home (reference) position. If X, Y, or Z values are specified, the machine moves to that intermediate position first, then moves to home. This is important for clearing the workpiece before the axes move to home.

G40 / G41 / G42 — Cutter Radius Compensation

Offsets the tool path by the tool's radius so you can program the actual part geometry instead of the tool center path. Most hobbyist CAM software handles this in the CAM output, so you may not see these in your programs.

G43 / G49 — Tool Length Offset

Applies (G43) or cancels (G49) a tool length compensation value from the tool table. Used on machines with automatic tool changers to account for different tool lengths.

G53 — Machine Coordinate Move

G53 is not a standalone command — it's prepended to a G00 or G01 move to make that single move use machine coordinates instead of work coordinates. Unlike G54–G59, G53 is non-modal: it only applies to the line it appears on, then the active work coordinate system takes over again on the next line.

This is most commonly used for safe retracts and tool changes, where you need to move to an absolute machine position regardless of where the work origin is set.

G54 – G59 — Work Coordinate Systems

Selects one of six available work coordinate systems. Each stores a different origin offset, letting you set up multiple parts or fixtures on the same machine. G54 is the default and most commonly used.

G80 – G89 — Canned Cycles

Canned cycles automate repetitive operations like drilling, tapping, and boring. Each cycle combines multiple motions into a single command. G80 cancels any active canned cycle.

Z = final depth, R = retract plane, Q = peck depth increment.

G90 / G91 — Absolute / Incremental Positioning

Controls how coordinates are interpreted.

Most CNC programs use G90 (absolute). G91 is useful for subroutines and specific operations like retracting the tool a fixed amount.

G92 — Set Position (Coordinate System Offset)

Sets the current position to the specified values without moving the machine. This effectively shifts the coordinate system. On GRBL machines, G92 is commonly used to set a temporary work origin.

G93 / G94 / G95 — Feed Rate Mode

Controls how the F (feed rate) value is interpreted.

G94 is the default on most machines. G93 is used with multi-axis machining; G95 with lathes.

M00 / M01 — Program Stop

M00 — Unconditional program stop. The machine halts and waits for the operator to press cycle start to resume.

M01 — Optional stop. Same as M00 but only stops if the operator has enabled the optional stop switch on the controller.

M02 / M30 — Program End

M02 — Ends the program. Stops spindle and coolant.

M30 — Ends the program and rewinds to the beginning. On most machines, M30 is preferred over M02 because it resets the program counter.

M03 / M04 / M05 — Spindle Control

M06 — Tool Change

Initiates a tool change. On machines with automatic tool changers, this swaps the current tool for the one specified by the T word. On manual machines, it pauses and waits for the operator to change the tool.

M07 / M08 / M09 — Coolant Control

F — Feed Rate

Sets the speed at which the tool moves during cutting (G01, G02, G03). The unit depends on the active unit mode: inches per minute with G20, or millimeters per minute with G21 (when in G94 mode).

Moves at 100 units/minute. Once set, the feed rate stays active until changed.

S — Spindle Speed

Sets the spindle rotation speed in RPM (revolutions per minute). Used with M03 or M04 to start the spindle.

Starts the spindle at 18,000 RPM clockwise.

T — Tool Select

Selects a tool from the tool magazine or turret. The tool is not loaded until M06 is called. Tool numbers correspond to positions in the machine's tool table.

N — Line Number

Optional line number for reference and program organization. Line numbers don't affect execution — they're labels for human readability and for use with GOTO commands on some controllers.

O — Program Number

Identifies the program with a unique number. Used on machines that store multiple programs. Typically appears as the first line of a program.

Comments

Comments are ignored by the controller and are used to document the program for human readers. The two common comment styles:

Parentheses comments are part of the G-code standard and work on most machines. Semicolon comments are common on GRBL-based machines and hobby controllers.