Printed from Kezuriba (kezuriba.net/en/nc/g84/)

G84

Machining center, LatheModal, group 09

Tapping cycle (right-hand thread)

⌨On machining centers

G84 X_ Y_ Z_ R_ P_ F_ K_

Cuts in with the spindle forward and reverses at the hole bottom to withdraw
Feed is spindle speed × pitch (feed per minute). Example: M10×1.5 at 500 min⁻¹ gives F750
How to choose between a floating tap holder (compensating chuck) and rigid (synchronized) tapping differs by machine. On FANUC-type controls, commanding M29 S_ before G84 is common (see M29)
Feed override is disabled during tapping (Siemens ISO)

Diagram: G84 motion (side view)

Taps in with feed with the spindle forward, reverses at the hole bottom and feeds out (right-hand thread). Feed = rpm × pitch. Figure shows G98 (rapid from R point to initial point).

◎On lathes: Face tapping cycle (lathe with live tooling)

The same number means something different on lathes (FANUC-type G-code system A). Group 10.

≠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	No M03/M04 is needed before G84 (the cycle starts and stops the spindle), and M29 is not used eitherOn Haas, S can be written on the G84 line, and J specifies the retract speed multiplier
Haas	Lathe	Group	09

📚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