Printed from Kezuriba (kezuriba.net/en/nc/g74/)

G74

Machining center, LatheModal, group 09

Left-hand tapping cycle (reverse tapping)

⌨On machining centers

G74 X_ Y_ Z_ R_ P_ F_ K_

Cuts in with the spindle in reverse and switches to forward at the hole bottom to withdraw. For left-hand threads
Feed is pitch × spindle speed (feed per minute). With feed per revolution, put the pitch directly in F
How to switch to rigid tapping differs by machine (M29, etc.; see the M29 entry)

Diagram: G74 motion (side view)

Taps in with spindle reverse, switches to forward at the hole bottom and feeds out (left-hand thread). Figure shows G98 (rapid from R point to initial point).

◎On lathes: End face grooving cycle / Z-direction deep hole peck drilling

The same number means something different on lathes (FANUC-type G-code system A). Group 00.

G74 R_ (retract amount);
G74 X(U)_ Z(W)_ P_ (X travel) Q_ (Z depth of cut) R_ F_

If X is omitted, it can be used as a Z-direction peck drilling (deep hole drilling) cycle at the center

Diagram (lathe): G74 (lathe), peck drilling in Z

Without X, it drills a deep center hole in Z, feeding Q at a time and rapid-retracting by the R amount of the first block each time to break the chip. With X and P, it becomes a face grooving cycle.

≠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	G74 X(U)_ Z(W)_ I_ K_ D_ F_ (one-block format; peck retract is Setting 22)

📚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
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