G-Code Complete Guide — A to Z

G-Code is the language used to control CNC machines. It tells the machine exactly how to move — where to go, how fast, and what to do. It is the Lingua Franca of CNC: used by CNC mills, lathes, routers, laser cutters, and 3D printers worldwide.

In order to make a part on a CNC machine, you write a G-Code program that describes every move the cutter must make. The machine's controller reads these instructions and moves the axes accordingly.

Armed with a solid understanding of G-Code, you can:

• Avoid running back to your CAM program when simple edits to the G-Code would do the job faster
• Understand and improve the G-Code your CAM program produces for better surface finish and cycle times
• Tweak your CAM post processor so it produces better code from the start
• Get a second opinion on CAM G-Code before finding out something is wrong at the machine
• Fix G-Code bugs quickly — a misplaced move that would otherwise require re-running the entire CAM workflow
• Create quick hand-written programs for simple parts without touching CAD/CAM at all
• Develop greater skill at the machine console, including MDI operation

CNC machines use a Right-Handed Coordinate System. Hold up your right hand with your index finger extended, thumb pointing up, and middle finger extended at right angles: your middle finger is X, index finger is Y, thumb is Z.

4-Axis, 5-Axis, and Rotational Axes

In addition to linear X, Y, Z axes, rotational axes can be added. By convention:

Rotational axes use degrees as their unit. Example: A90 rotates the 4th axis to 90°.

Expressing Coordinates in G-Code

Simply take the axis letter and add the value. Spaces are optional:

Absolute vs. Relative Coordinates

Example — cutting a 1″ square using relative mode (G91):

Offsets

Offsets are a way to shift the coordinate origin. Work Offsets (G54–G59) let you define multiple "Part Zeros" on the machine table at the same time — for example, to machine two identical parts held in separate vises without changing the program.

G-Code is not perfectly standardized. Different CNC controllers implement different dialects. The most common dialects are Fanuc (professional shops) and Mach3/LinuxCNC (hobbyists). Key differences include:

• Supported G-Codes: Not all controllers support all G-Codes. Early lathe controls often lack G71 roughing cycles.
• G-Code mappings: The same function may use different code numbers on different controllers.
• Formatting: Some controllers require G00, others accept G0. Some require decimal points: "1." vs "1.0" vs "1".
• Parameters: The letters used to pass additional information to a G-Code can vary between dialects.
• Macro Programming: Fanuc Macro B is the most common standard, but support varies widely.

Post Processors

If you use CAM software, it has a Post Processor (or "Post") that converts geometry moves into the specific G-Code dialect your machine needs. The Post is what ensures your CAM output is compatible with your controller. If you frequently make the same hand edits to your G-Code output, it's worth investigating whether a Post change would eliminate that work permanently.

Modal Behavior

G-Code is a modal language. Many commands set a "mode" that stays active until you change it. For example, once you issue G01 (feed motion), the machine stays in feed motion mode. You don't need to repeat G01 on every line — only when you want to change to a different mode.

MDI (Manual Data Input) lets you type G-Code commands directly into the CNC controller for immediate execution — no program file needed. Think of it as giving the machine orders one line at a time, exactly like a manual mill with digital readouts and power feeds on every axis.

Basic MDI Workflow

MDI Quick Reference

A line of G-Code is called a Block. A complete G-Code program is made of many blocks executed in sequence from top to bottom.

A Minimal G-Code Program

Block Structure Elements

Word Address Format

Every letter in G-Code is a Word. The number following it is its Address. For example: X1.5 — X is the word, 1.5 is the address. The letter always tells the controller what kind of information is coming next, and the number tells it the value.

Order of Execution Within a Block

Words in a block do not necessarily execute left to right. The controller has a defined order of operations: set feedrate mode → set feedrate → set spindle speed → select tool → change tool → spindle on/off → coolant → motion. If you are unsure about the order, put commands in separate blocks to guarantee sequence.

Comments

Anything inside parentheses is a comment and is completely ignored during execution:

Feedrate — The F Word

The F word sets the cutting speed in inches per minute (IPM) or mm/min depending on units mode. The feedrate is modal — set it once and it stays until you change it:

Spindle Speed — The S Word

The S word sets spindle RPM. Use it together with M03 (CW) or M04 (CCW). Both S and F are modal:

Interpolated Moves

When you specify multiple axes in one block, all axes move simultaneously and arrive at the destination at the same time — this is called interpolated motion. The controller coordinates their speeds automatically:

Older Machine Warning — "Dog Leg" G00

Older controllers may "dog leg" G00 — moving one axis at a time instead of a coordinated straight line. Be very careful programming G00 moves on older machines if there are any obstacles in the path.

Defining an Arc: Two Methods

Every arc needs three things: a starting point (current position), an ending point (XYZ), and the center location. There are two ways to specify the center:

Method 1 — IJK (Relative Offsets from Start Point)

I, J, K are the distances from the starting point to the center of the arc, along X, Y, Z respectively. Add I to start-X to get center-X, add J to start-Y to get center-Y.

Method 2 — R (Radius)

Simply specify the radius with the R word. Easier to write, but note: full circles cannot be programmed with R (ambiguous). For arcs over 180°, use a negative R to force the longer path.

Full Circles — Same Start and End Point

A full circle has identical start and end points. Must use IJK (not R — infinitely ambiguous with R):

Common Problem: Absolute vs Relative IJK

The most common configuration error when setting up a CAM post or simulator is mismatching absolute vs relative IJK. If your backplot shows giant circles instead of the expected toolpath, check this setting first. IJK is relative (offset from start point) by default on most Fanuc-style controllers, but some controllers use absolute (actual center coordinates).

Arcs for Better Toolpaths

Whenever a cutter changes direction abruptly (especially 90°), it creates stress and can leave marks in the finish. Program a small arc at each corner rather than a sharp direction change. Even a tiny radius allows the controller to avoid instantaneous direction reversal and will improve surface finish and tool life.

Arcs are also the best way to enter a cut — gradually ramping in with an arc instead of plunging straight down greatly reduces cutting forces and extends tool life.

A helix is a circular arc that simultaneously moves in a third axis (Z). Helical interpolation is used for thread milling, ramping into a pocket, and interpolating large holes. You add a Z value to a G02/G03 block to create helical motion:

In this thread-milling example, each arc block moves the cutter 0.018" deeper in Z while completing one revolution — creating one thread pitch per pass.

Part Zero (also called Work Zero or Program Zero) is the X0 Y0 Z0 origin point your G-Code program refers to. Before running any program, you must tell the machine where Part Zero is in relation to the machine's own coordinate system.

Where to Put Part Zero

Machine Coordinates vs Work Coordinates

Machine Coordinates are fixed — they are set when you home the machine. Work Coordinates are what your G-Code program uses. You establish Work Coordinates by "touching off" — finding the edge of your part and telling the machine that location is X0, Y0, or Z0.

Touch Off Methods

• Paper method: Use a thin piece of paper (cigarette paper works well) dampened with oil. Jog the spinning cutter until it just moves the paper. Adjust for paper thickness.
• Gage block: Use a precision gage block between the stationary cutter and the workpiece surface. Jog until the block just fits with slight drag.
• Edge finder: A spinning probe that kicks off-center when it touches a workpiece edge, giving a precise X or Y zero.
• 3D Taster (Haimer): A mechanical probe that precisely finds edges and centers. Very fast and accurate.
• Renishaw probe: Electronic touch probe. Fastest and most accurate — used in production environments.

Multiple Work Coordinate Systems

G54 through G59 each define an independent Work Coordinate System. This lets you machine multiple identical parts held in separate vises — each vise gets its own Work Offset. The same program runs against each offset to machine each part.

Most CNC programs use more than one tool. Tool change codes serve two purposes: (1) physically change the tool in the spindle, and (2) load the Tool Length Offset — a value that compensates for the fact that different tools have different lengths.

Mill Tool Change — T + M06

Tool Length Offsets

Every tool has a different length. The Geometry Offset (stored in the tool table) compensates for the overall length difference. The Wear Offset is a fine-tuning adjustment for gradual tool wear and allows the machinist to hit exact tolerances without editing the program.

Use G43 to apply a tool length offset (H word references the offset register):

Lathe Tool Change (Fanuc Style)

On lathes, no M06 is needed — the tool changes as soon as the T word executes. Fanuc combines tool number and wear offset in one T command:

A basic CNC lathe uses only two axes: Z (parallel to the spindle) and X (perpendicular to the spindle). The same G00, G01, G02, G03 motion codes are used, but without Y.

Diameter vs Radius Mode

Most lathes operate in Diameter Mode by default: X values represent the diameter of the part, not the distance from centerline. A part with a 2" diameter is programmed as X2.0, even though the tool is only 1.0" from the centerline. Check your controller's manual to verify which mode it defaults to.

Part Zero on Lathe Programs

The X-axis zero is always the spindle centerline. For Z, the three common options are:

• End of finished part — most common; easy to relate dimensions to the print
• Chuck jaw face — useful when machining both ends
• Chuck face — least useful, rarely matches the actual part position

Simple Lathe Program Example

Many CNC lathe controllers support automatic chamfer and corner rounding as part of a G01 move. Instead of programming a separate G02/G03 arc, you add a C (chamfer) or R (radius) word to the G01 block and the controller inserts the feature automatically at the transition.

Use C for a chamfer and R for a radius. The sign (positive or negative) depends on which direction you are moving and what the next direction will be — consult your controller's chart or simply try both and verify in your simulator.

GCodex G-Code guide · learn g-code · g-code tutorial · g-code course · G00 G01 G02 G03 · CNC g-code reference · circular arcs gcode · tool changes g-code · lathe g-code · MDI cnc · g-code for beginners · free g-code course · gcode viewer · ncviewer alternative · gcodex.tech