Printed from Kezuriba (kezuriba.net/en/nc/g28/)

G28

Machining center, LatheOne-shot, group 00

Automatic return to reference point (zero return)

⌨Format and notes

G91 G28 Z0 (machining center) / G28 U0 W0 (lathe)

The commanded coordinate is an intermediate point: the machine first rapids there, then returns to the reference point
Writing G28 X0 Y0 Z0 under G90 passes through the work origin. To avoid creating an intermediate point, use G91 G28 Z0 (U0/W0 on lathes)
On machining centers it is safer to raise Z first, then return X and Y (Mitsubishi machining center material)
On lathes, returning X(U) and Z(W) one after the other in separate blocks reduces the risk of interference (Mitsubishi lathe material)
Axes that are not written do not return

Diagram: G28: return to reference point via intermediate point

The coordinates commanded in G28 are the intermediate point on the way. The axes rapid to it first, then return to the reference point. Writing Z0 in G90 passes through the workpiece top, so return Z straight up with G91 G28 Z0.

≠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	Notes	G28 with no axes returns all axes to the machine origin at onceHaas returns all axes when none is specified. On FANUC-type controls (Siemens ISO), only the specified axes return

📚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
Mitsubishi Electric — The Basics of CNC Machining Programming (for Lathe) e-Learning material (PDF, BNP-C8027-688) 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
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
National Institute of Standards and Technology (NIST), USA — The NIST RS274NGC Interpreter – Version 3 (NISTIR 6556, 2000) nvlpubs.nist.gov
Ministry of Health, Labour and Welfare (MHLW), Human Resources Development Bureau, Office of the Councillor for Skills Evaluation — Human resource development manual using the practical exam tasks of the Grade 3 Skilled Worker Test: CNC lathe work (March 2018) waza.mhlw.go.jp