Printed from Kezuriba (kezuriba.net/en/nc/g92/)

G92

Machining center, LatheOne-shot, group 00

Coordinate system setting (assigns coordinate values to the current position)

⌨On machining centers

G92 X_ Y_ Z_

The axes do not move; the coordinate system is shifted so that the current position becomes the specified coordinates
Mixing G92 into a workflow that uses G54–G59 shifts all coordinate systems and gets confusing. Also check how to cancel it, e.g. with G92.1
On Siemens ISO, G92 S_ also sets the spindle speed limit

Diagram: Machine zero and work zero (coordinate systems)

G92 X_ Y_ doesn't move the axes; it redefines the origin so the current tool position takes the specified coordinate values. Mixing it with G54–G59 makes offsets hard to follow.

◎On lathes: Thread cutting cycle (single canned cycle, G-code system A)

The same number means something different on lathes (FANUC-type G-code system A). Group 01.

G92 X(U)_ Z(W)_ F_ (lead) (R_ for taper thread)

Write many lines changing only X, cutting in a little at a time to finish the thread (straight infeed each pass)
F is the lead. On many machines the feed override is disabled during threading
System B uses G78 and system C uses G21 (Siemens ISO T). G92 in systems B/C is coordinate system setting

Diagram (lathe): the 4 motions of G92 (lathe)

4 motions: ① infeed ② cut thread ③ retract ④ return. F is the lead, not the pitch. Repeat blocks changing only X to cut the thread deeper step by step.

≠Differences between controls and machines

The same code can be written or assigned differently depending on the CNC control and the machine builder. Always check your machine’s manual.

Source	Machine	Item	Detail
Haas	Machining center	Meaning	Sets the shift amount for all work coordinate systems (G54–G59, G110–G129)On Haas, the shift amount is shown below the work offset screen and is cleared by power-up and zero return
Haas	Lathe	Format	Taper is I_, and Q is the start angleHaas switches the chamfer at the end of the thread with Setting 95/96 and M23/M24

📚Sources

The meaning shown agrees in at least two sources (agreement confirmed). Explanations are written in our own words.

Siemens AG — SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D Programming Manual ISO Milling, 04.2007 Edition (6FC5398-7BP10-0BA0) cache.industry.siemens.com
Haas Automation, Inc. — G-code, M-code, and Setting (per-code explanation pages) haascnc.com
Haas Automation, Inc. — Mill Operator's Manual – 17 Mill G-Codes (online version) haascnc.com
National Institute of Standards and Technology (NIST), USA — The NIST RS274NGC Interpreter – Version 3 (NISTIR 6556, 2000) nvlpubs.nist.gov
Siemens AG — SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D Programming Manual ISO Turning, 04.2007 Edition cache.industry.siemens.com
Haas Automation, Inc. — Lathe Operator's Manual – 16 Lathe G-Codes (online version) haascnc.com