G-code / M-code

Quick reference

Motion

G00Rapid positioning
Moves the tool at max speed to the coordinate. Positioning only — never use it to cut.
Syntax
```
G00 X__ Z__
```
Example
```
G00 X50. Z2.  (approach the part)
```
G01Linear interpolation
Straight-line move at feed rate F. The most common straight-cut mode.
Syntax
```
G01 X__ Z__ F__
```
Example
```
G01 Z-30. F0.2  (turn 30 mm in Z)
```
G02Clockwise circular interpolation
Arc clockwise. Use I/K (offset from start to arc center) or R (radius).
Syntax
```
G02 X__ Z__ I__ K__ F__  or  G02 X__ Z__ R__ F__
```
Example
```
G02 X40. Z-10. R5. F0.15
```
G03Counter-clockwise circular interpolation
Same as G02 but counter-clockwise.
Syntax
```
G03 X__ Z__ R__ F__
```
Example
```
G03 X30. Z-15. R8. F0.15
```
G04Dwell (pause)
Pauses for the time given in X (seconds) or P (milliseconds). Useful at groove bottoms.
Syntax
```
G04 X__  or  G04 P__
```
Example
```
G04 X0.5  (half a second)
```

Plane

G17XY plane
Selects the XY plane for circular interpolation. Default on milling machines.
Syntax
```
G17
```
G18ZX plane
Selects the ZX plane. Default on lathes.
Syntax
```
G18
```
G19YZ plane
Selects the YZ plane. Used on 4/5-axis mills.
Syntax
```
G19
```

Unit

G20Inches
Sets units to inches.
Syntax
```
G20
```
G21Millimeters
Sets units to millimeters.
Syntax
```
G21
```

Reference

G27Reference return check
Checks that the current coordinates match the reference point. Lights the zero lamp.
Syntax
```
G27 X__ Z__
```
G28Return to machine zero
Returns the commanded axes to the reference point through an intermediate point.
Syntax
```
G28 X__ Z__
```
Example
```
G28 U0 W0  (incremental direct return)
```
G29Return from reference point
Moves from the reference point to the intermediate point and then to the destination.
Syntax
```
G29 X__ Z__
```
G302nd/3rd/4th reference point
Moves to a secondary reference point set by parameter.
Syntax
```
G30 P__ X__ Z__
```

Thread

G32Single-pass threading
Single-pass threading (straight or tapered). F sets the thread pitch.
Syntax
```
G32 X__ Z__ F__
```
Example
```
G32 Z-25. F1.5  (1.5 mm pitch thread)
```

Compensation

G40Cancel cutter compensation
Turns G41/G42 off. Program it before leaving the profile.
Syntax
```
G40
```
G41Left compensation
Offsets the toolpath one tool radius to the left, viewed along the feed direction.
Syntax
```
G41 D__  or  G41 (lathe uses insert nose radius)
```
G42Right compensation
Same as G41 but to the right of the feed direction. Most common on external turning.
Syntax
```
G42
```

Spindle

G50Spindle speed limit (lathe)
Sets the maximum RPM while G96 (constant surface speed) is active.
Syntax
```
G50 S__
```
Example
```
G50 S3000
```
G96Constant surface speed (lathe)
The machine adjusts RPM automatically with diameter to keep Vc (m/min) constant.
Syntax
```
G96 S__
```
Example
```
G50 S3000
G96 S200
```
G97Constant RPM
S directly sets spindle speed in RPM. Required for threading.
Syntax
```
G97 S__
```
Example
```
G97 S1200
```

Work zero

G54Work zero 1
Activates work coordinate system 1. Goes up to G59.
Syntax
```
G54
```

Lathe cycle

G70Finishing cycle
Re-runs the profile defined between P (start line) and Q (end line) in a single fine pass.
Syntax
```
G70 P__ Q__
```
Example
```
G70 P100 Q200
```
G71Longitudinal roughing
Removes material parallel to Z in automatic passes. U depth per pass, R retract, U/W finishing stock.
Syntax
```
G71 U__ R__ ;  G71 P__ Q__ U__ W__ F__
```
Example
```
G71 U2. R1.
G71 P100 Q200 U0.4 W0.1 F0.25
```
G72Facing roughing
Same as G71 but passes parallel to X (stepped facing).
Syntax
```
G72 W__ R__ ;  G72 P__ Q__ U__ W__ F__
```
G73Pattern repeating
Ideal for forged/cast parts: repeats the P–Q profile shifting it in X and Z until the final size.
Syntax
```
G73 U__ W__ R__ ;  G73 P__ Q__ U__ W__ F__
```
G74Face peck drilling
Axial peck drilling on the lathe: drills, retracts to break the chip, and continues.
Syntax
```
G74 R__ ;  G74 Z__ Q__ F__
```
G75Radial grooving
Cuts radial grooves in X with automatic retract to break chips.
Syntax
```
G75 R__ ;  G75 X__ Z__ P__ Q__ F__
```
G76Automatic threading cycle
Threads in several passes computing decreasing depth and insert angle.
Syntax
```
G76 P(mmrra) Q__ R__ ;  G76 X__ Z__ P__ Q__ F__
```
Example
```
G76 P020060 Q100 R0.02
G76 X28.16 Z-24. P920 Q200 F1.5
```

Mill cycle

G80Cancel canned cycle
Turns off any active G81–G89 cycle.
Syntax
```
G80
```
G81Simple drilling
Feeds down to Z, retracts in rapid. No chip breaking.
Syntax
```
G81 X__ Y__ Z__ R__ F__
```
G83Peck drilling
Deep drilling with programmed retracts to break the chip.
Syntax
```
G83 X__ Y__ Z__ Q__ R__ F__
```
G84Tapping
Tapping cycle (rigid or floating).
Syntax
```
G84 X__ Y__ Z__ R__ F__
```
G98Return to initial plane
In canned cycles, returns the tool to the initial Z plane.
Syntax
```
G98
```
G99Return to R plane
In canned cycles, returns only to the R plane.
Syntax
```
G99
```

Mode

G90Absolute coordinates
Coordinates measured from the work zero.
Syntax
```
G90
```
G91Incremental coordinates
Coordinates relative to the current position.
Syntax
```
G91
```

Feed

G94Feed per minute
F in mm/min. Default on mills.
Syntax
```
G94
```
G95Feed per revolution
F in mm/rev. Default on lathes.
Syntax
```
G95
```