LinuxCNC G71

G71 is a LinuxCNC lathe roughing cycle that removes material in layers along Z to rough-cut a profile defined in a subroutine. The subroutine number is given by Q, and optional X and Z set the starting position, D the remaining distance, I the cutting increment, and R the retracting distance. It requires the ZX plane and is intended to leave material for a finishing cycle.

Source checked15/15 values · 2026-10-26

Specification

1 source

Language	gcode
Code	G71
Group	Lathe roughing cycle
Syntax	G71 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

G71 removes layers of material while traversing in the Z direction; the profile's Z coordinate must be monotonically changing.
The profile subroutine may contain G0, G1, G2 and G3 motion commands; all other commands, including feed and speed settings, are ignored, and G0 commands are interpreted as G1.
An optional A number on a motion command inserts a fillet at that endpoint, and an optional C number inserts a chamfer; a too-large fillet radius can fail with a non-monotonic path error.
In absolute mode, U (for X) and W (for Z) can be used as incremental displacements.
D keeps a distance from the final profile to allow material to remain for finishing.
If X or Z are used, a rapid move to that position is made before cutting; after the profile is cut, the tool stops at the end of the profile including the D distance.
It is an error if no subroutine Q exists, if the profile is not monotonic in Z or X, if the ZX plane is not selected, or if G41/G42 cutter compensation is active.
The document notes that the G71 roughing cycle is currently somewhat fragile; it cites issues #707 and #1146.