LinuxCNC G72 Lathe Facing Roughing Cycle

G72 is a LinuxCNC lathe roughing cycle for facing: it removes material by traversing along the X axis, following a profile defined in a subroutine selected by Q. X and Z set the start position, D leaves distance for finishing, I sets the cutting increment, and R sets the retracting distance. The profile path must change monotonically in X.

Source checked15/15 values · 2026-10-26

Specification

1 source

Language	gcode
Code	G72
Group	Lathe roughing cycles
Syntax	G72 Q- <X-> <Z-> <D-> <I-> <R->
Dialect	LinuxCNC

Parameters

Name	Description
Q	The subroutine number.
X	The starting X position, defaults to the initial position.
Z	The starting Z position, defaults to the initial position.
D	The remaining distance to the profile, defaults to 0.
I	The cutting increment, defaults to 1.
R	The retracting distance, defaults to 0.5.

Study notes

G72 removes material while traversing the X axis; the document calls it the facing cycle.
The direction of travel is the same as in the path given in the subroutine selected by Q.
The Q subroutine may contain G0, G1, G2 and G3 motions; all other commands are ignored, including feed and speed settings. G0 commands are interpreted as G1.
Profile motion commands may include an optional A- number for a fillet radius or a C- number for a chamfer at the motion endpoint.
In absolute mode, U (for X) and W (for Z) can be used as incremental displacements.
G72.1 does not cut pockets; G72.2 cuts only after the first pocket and continues where G72.1 stopped.
The normal G72 cycle cuts the entire profile in one cycle.
After cutting, the tool stops at the end of the profile plus the distance specified by D.
D keeps a distance from the final profile so material remains for finishing.
The document refers to plane selection as [gcode:g17-g19.1]; the ZX plane must be selected before this cycle.

Safety

The document warns that the G71 and G72 roughing cycles are currently somewhat fragile (issues #707 and #1146).
Cutter compensation (G41/G42) must be off when G72 is executed; the cycle reports an error if it is active.
A non-monotonic profile path in X causes an error for G72.
The ZX plane must be selected before G72; otherwise the cycle errors.