Complete G-Code List: CNC Programming Reference with Examples

Complete G-Code List: CNC Programming Reference

G-code (Geometric code) is the programming language that tells a CNC machine where to move, how fast to move, and what path to follow. Think of it as giving your machine a set of coordinates — and it moves the tool to those coordinates with perfect precision every time.

A single G-code line breaks down like this:

G01 X100 Y50 Z-5 F200

Part	Meaning
G01	Command: linear feed move
X100 Y50 Z-5	Target coordinates
F200	Feed rate: 200 mm/min

This page covers every G-code you’ll ever need — from the 15 essential codes you’ll use daily to the full reference table organized by functional group, plus controller-specific differences and real mistakes to avoid. Bookmark this page and come back every time you write a CNC program.

---

Essential G-Codes Every CNC Programmer Must Know

You can write 90% of CNC programs with just these 15 codes. Master these first the rest will follow naturally.

Code	Function	Example	When You Use It
G00	Rapid positioning	G00 X100 Y50	Moving to a position without cutting
G01	Linear feed (cutting)	G01 X100 F200	Cutting a straight line
G02	Arc clockwise	G02 X100 Y50 R25	Cutting an arc or fillet
G03	Arc counterclockwise	G03 X100 Y50 R25	Cutting an arc in reverse
G17	XY plane (default)	G17	Milling operations
G20	Inch mode	G20	Programming in inches
G21	Metric mode	G21	Programming in millimeters
G40	Cancel cutter comp	G40	Turning off radius offset
G43	Tool length offset (+)	G43 H1	Activating a tool’s length
G54	Work offset 1	G54	Picking your part zero
G81	Simple drill cycle	G81 R2 Z-10 F150	Drilling a standard hole
G83	Peck drill cycle	G83 R2 Z-25 Q5 F120	Drilling a deep hole
G90	Absolute positioning	G90	Coordinates from part zero
G91	Incremental positioning	G91	Coordinates from current position
G94	Feed per minute	G94	Standard feed rate mode

G-Code Decision Flowchart

Not sure which motion code to use? Follow this simple decision tree:

graph TD
    A{What do you want<br>the tool to do?} --> B{Is the tool<br>cutting material?}
    B -->|No, just positioning| C[Use **G00** Rapid]
    B -->|Yes, cutting| D{What shape?}
    D -->|Straight line| E[Use **G01** Linear Feed]
    D -->|Arc or circle| F{Which direction?}
    F -->|Clockwise| G[Use **G02**]
    F -->|Counterclockwise| H[Use **G03**]
    C --> I[Keep G00 moves<br>above the workpiece]
    E --> J[Set feed rate F<br>before cutting]

Modal vs One-Shot Codes

G-codes come in two types. Understanding the difference between them prevents crashes.

Modal codes stay active until you change them. You write them once and they affect every following line:

G90 G01 X50 F200  ; G90 and G01 are now active
X100               ; Still G90 + G01 → absolute linear move to X100
Y50                ; Still G90 + G01 → absolute linear move to Y50

One-shot codes only affect the line they are on:

G04 P1000          ; Dwell for 1 second — only this line
G81 R2 Z-10 F150   ; Drill cycle — cancels after G80

💡 Pro tip: Always set your mode explicitly at the start of each program. Never assume what mode the previous program left the machine in. This is called a safety block and it saves tools: G90 G94 G17 G54

---

Complete G-Code Reference Table

All G-codes listed by functional group. Most groups are modal — once selected the code stays active until another code in the same group replaces it.

Group 01: Motion Codes

Code	Description	Modal	Example
G00	Rapid positioning	Yes	G00 X100 Y50
G01	Linear interpolation (feed)	Yes	G01 X100 F200
G02	Circular interpolation CW	Yes	G02 X100 Y50 R25
G03	Circular interpolation CCW	Yes	G03 X100 Y50 I25 J0
G04	Dwell (pause)	No	G04 P1000 (wait 1000ms)
G09	Exact stop check	No	G09 G01 X100

For full circles always use IJK format not R. The R method cannot create a complete circle. IJK defines the center point relative to the start position giving you full 360-degree control.

Group 02: Plane Selection

Code	Description	Modal	Default Machine
G17	XY plane	Yes	Mills
G18	XZ plane	Yes	Lathes
G19	YZ plane	Yes	Rare

Group 03: Distance Mode

Code	Description	Modal	Example
G90	Absolute positioning	Yes	G90 G01 X50 → move to X=50
G91	Incremental positioning	Yes	G91 G01 X50 → move +50 from here

G90 (Absolute)                    G91 (Incremental)
───┬───┬───┬───┬───              ───┬───┬───┬───┬───
 0  25  50  75  100               0  25  50  75  100
         ↑ ← Tool at 25                ↑ ← Tool at 25
    G90 X75 → Tool goes TO 75     G91 X50 → Tool moves +50 to 75

🚨 Beginner mistake: Forgetting to switch back from G91. If you use G91 in a subprogram and do not end with G90 your next tool position will shift by the incremental amount. Always end subprograms with G90 before returning to the main program line.

Group 05: Feed Rate Mode

Code	Description	Modal	Notes
G94	Feed per minute	Yes	Standard for mills
G95	Feed per revolution	Yes	Standard for lathes

Group 06: Units

Code	Description	Modal
G20	Inch mode	Yes
G21	Metric mode (millimeters)	Yes

Group 07: Cutter Compensation

Code	Description	Modal	When to Use
G40	Cancel cutter comp	Yes	Default — no offset
G41	Cutter compensation left	Yes	Tool is left of the profile
G42	Cutter compensation right	Yes	Tool is right of the profile

G41 D1 G01 X50 F200  ; Activate comp for tool 1 offset left
G40 G00 Z5           ; Cancel comp before retracting

🚨 Beginner mistake: Activating G41 or G42 without a G01 move on the same line causes an alarm. Always pair activation with a linear feed move so the controller can calculate the offset direction.

Group 08: Tool Length Offset

Code	Description	Modal
G43	Tool length offset (positive)	Yes
G44	Tool length offset (negative)	Yes
G49	Cancel tool length offset	Yes

Group 09: Canned Cycles (Drilling)

Code	Description	Example	Best For
G73	Chip breaking (peck)	G73 R2 Z-25 Q5 F120	Deep holes small chips
G81	Simple drilling	G81 R2 Z-10 F150	Standard hole
G82	Spot drill with dwell	G82 R2 Z-5 P500 F100	Counterbores and spotfaces
G83	Peck drilling (full retract)	G83 R2 Z-40 Q8 F120	Deep holes clear chips
G84	Rigid tapping	G84 R2 Z-20 F500	Threading holes
G85	Boring (feed out)	G85 R2 Z-30 F120	Precision bores
G86	Boring (rapid out)	G86 R2 Z-30 F120	Rough boring
G89	Boring with dwell	G89 R2 Z-30 P500 F120	Bottom finish

Cancel any canned cycle with: G80

Group 12: Work Offsets

Code	Description	Used For
G54	Work offset 1	Primary part position
G55	Work offset 2	Second part or operation
G56	Work offset 3	Third setup
G57	Work offset 4	Fourth setup
G58	Work offset 5	Fifth setup
G59	Work offset 6	Sixth setup

Other Useful G-Codes

Code	Description	Notes
G28	Return to home position	G28 G91 Z0 — safe retract then home
G30	Return to 2nd home	Tool change position
G50	Max spindle speed (lathe)	G50 S3000 limits to 3000 RPM
G92	Set coordinate offset	Use sparingly — prefer G54
G96	Constant surface speed (lathe)	G96 S150 M03
G97	Cancel CSS (lathe)	G97 S1200 M03
G98	Return to initial Z level	Safer for canned cycles (clears obstacles)
G99	Return to R plane	Faster for canned cycles

---

G-Code by Controller: What’s Different

Most G-codes are universal but each controller has its own quirks. Here is what to watch for when switching between machines:

Code	Fanuc	Haas	GRBL	LinuxCNC
G28	Standard	Same as Fanuc	Not supported	Works
G30	2nd reference point	Same	Not supported	G28.1
G43	Tool length on	Same	Not needed	Same
G52	Local coordinate	Same	Limited	Limited
G53	Machine coordinates	Same	Works	Works
G73	Chip breaking	Same	Limited	Works
G84	Rigid tap	Same	Not supported	Works
G96	CSS	Same	Not supported	Works

💡 Rule of thumb: Fanuc is the industry standard. Haas is very similar with minor extensions. GRBL is a simplified subset of about 30 codes. LinuxCNC is the most flexible but uses unique syntax for advanced features like parametric programming.

---

Common G-Code Mistakes Beginners Make

1. Using G00 When the Tool is in the Material

; ❌ WRONG — G00 is rapid speed and will crash
G00 Z-5 F100

; ✅ RIGHT — use G01 to feed into material
G01 Z-5 F100

What happened: The tool plunged into the workpiece at maximum machine speed. A 6mm end mill does not survive this. Neither does the workpiece.

2. Forgetting to Cancel G91 After a Subprogram

; Subprogram using incremental mode
O1000
G91 G01 X10
Y10
M99

; Back in main program — G91 is STILL ACTIVE!
; Your next G90 move is now interpreted as incremental.

Fix: Always end subprograms by switching back to absolute mode:

O1000
G91 G01 X10
Y10
G90  ; Switch back BEFORE returning
M99

3. Activating Cutter Compensation Without a Feed Move

; ❌ WRONG — this triggers an alarm
G41 G00 X50

; ✅ RIGHT — activate compensation with a feed move
G41 G01 X50 F200

Why it happens: Cutter compensation needs a feed move to calculate which direction to offset the tool path. A rapid move at G00 speed does not provide enough information.

4. Confusing G98 vs G99 in Canned Cycles

G81 R2 Z-10 F150              ; Returns to R plane (Z2) by default
G98 G81 R2 Z-10 F150          ; Returns to initial Z level (safer)
G99 G81 R2 Z-10 F150          ; Returns to R plane (faster)

Which one should you use: G98 when you need to clear clamps or obstacles above the part. G99 when the surface is open and you want to save cycle time.

5. Using G92 Instead of G54 for Work Offsets

; ❌ WRONG — G92 is temporary lost on reset
G92 X0 Y0 Z0

; ✅ RIGHT — use G54 work offset
G54 G00 X0 Y0 Z0

Why it matters: G92 shifts the coordinate system temporarily. If you hit the reset button or restart the program G92 is gone and your zero position moves. G54 stores the offset permanently in the controller memory.

---

G-Code Quick Reference: Cheatsheet

A print-friendly quick reference for daily use:

MOTION               MODAL   EXAMPLE
G00 Rapid            Yes     G00 X100
G01 Linear Feed      Yes     G01 X100 F200
G02 Arc CW           Yes     G02 X100 R25
G03 Arc CCW          Yes     G03 X100 I25
G04 Dwell            No      G04 P1000

PLANE                MODAL   DEFAULT
G17 XY               Yes     Mills
G18 XZ               Yes     Lathes
G19 YZ               Yes     Rare

MODE                 MODAL   BEHAVIOR
G90 Absolute         Yes     Go TO coordinate
G91 Incremental      Yes     Move BY amount

UNITS                MODAL
G20 Inches           Yes
G21 Millimeters      Yes

CUTTER COMP          MODAL
G40 Cancel           Yes
G41 Left             Yes
G42 Right            Yes

TOOL OFFSET          MODAL
G43 Length +         Yes
G49 Cancel           Yes

CANNED CYCLES        SYNTAX
G81 Simple drill     G81 R2 Z-10 F150
G83 Peck drill       G83 R2 Z-40 Q8 F120
G84 Rigid tap        G84 R2 Z-20 F500
G80 Cancel           Always close with G80

WORK OFFSETS         RANGE
G54-G59              Six part zero positions

SAFETY BLOCK         Always start with this:
G90 G94 G17 G54      (absolute, feed/min, XY plane, offset 1)

---

Frequently Asked Questions

How many G-codes are there in total?

About 100 G-codes exist across all controller dialects. Most programmers only use 15 to 20 regularly. The full Fanuc set includes roughly 85 codes. GRBL supports about 30. LinuxCNC supports the most including parametric macros and NURBS interpolation.

What is the difference between G-code and M-code?

G-code controls geometry — where the tool moves and what path it follows. M-code controls machine functions — spindle on or off, coolant flow, tool changes, and program flow.

G01 X100 F200  ; G-code: move the tool along a path
M03 S3000      ; M-code: start the spindle
M08            ; M-code: turn on coolant
G00 Z5         ; G-code: rapid retract
M30            ; M-code: end the program

Do I need to memorize all G-codes?

No. Every CNC programmer keeps a reference sheet at their machine. The skill is not memorizing every code number. The skill is understanding what type of operation you need and which code group controls it. With practice the 15 essential codes become automatic. For everything else you bookmark this page and come back when you need it.

---

What’s Next?

Now that you have the complete G-code reference learn how each code works in practice:

• G00 and G01: Rapid and Linear Moves Explained
• G90 vs G91: Absolute vs Incremental Positioning
• Complete M-Code List Reference
• G81 Drilling Cycle Explained