Printed from Kezuriba (kezuriba.net/en/nc/g90/)

G90

Machining center, LatheModal, group 03

Absolute command

⌨On machining centers

G90 G00 X_ Y_

Coordinate values are written as positions from the origin of the current work coordinate system
I/J/K (arc center) remain incremental even under G90 (NIST)

Diagram: Writing the same move in absolute (G90) and incremental (G91)

The same path from the origin through ①→②→③ is written in G90 as positions from the origin and in G91 as moves from the current position. In G91, axes that do not move need not be written.

◎On lathes: OD/ID 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.

G90 X(U)_ Z(W)_ F_ (R_ for taper)

One command performs four motions: infeed, cut, relief, and return. Write consecutive lines changing only X to take multiple passes
In system A, absolute/incremental is distinguished by address (X, Z versus U, W), not by G90/G91
System B uses G77 and system C uses G20 for the same function (Siemens ISO T)

Diagram (lathe): the 4 motions of G90 (lathe)

One block does 4 motions: ① infeed ② cut in Z ③ retract ④ return (the light orange area is cut in this one pass). Repeat blocks changing only X to cut 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	Lathe	Format	Taper is I_ (radius value)R on FANUC-type controls (Siemens ISO T), I on Haas
Haas	Lathe	Notes	The absolute/incremental G-codes on Haas lathes are G390/G391

📚Sources

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

Mitsubishi Electric — The Basics of CNC Machining Programming (for Machining center) e-Learning material (PDF) mitsubishielectric.com
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. — 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
Saitama University, Faculty of Engineering, Department of Mechanical Engineering, practical training — Machining center program 2019 (training NC program O19-0101, with comments) jisshu.mech.saitama-u.ac.jp
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. — G-code, M-code, and Setting (per-code explanation pages) haascnc.com
Haas Automation, Inc. — Lathe Operator's Manual – 16 Lathe G-Codes (online version) haascnc.com