Haas Lathe · G-code
G76 Threading Cycle, Multiple Pass
Cuts a complete thread from one line: first pass depth, total height, infeed angle and lead.
What G76 does on a Haas lathe
G76 calculates every pass of a thread from a single Haas block. K is the thread height (per side), D is the first-pass depth, F is the lead and A is the tool angle used for compound infeed. Passes get progressively lighter.
P selects the cutting method (P1–P4 — single or alternating flank, constant amount or constant depth). I adds taper for pipe threads.
G76 format
| Address | Meaning |
|---|---|
X | Minor (OD) or major (ID) diameter at the finish |
Z | Thread end |
K | Thread height, per side |
D | First pass depth |
F | Lead (1 ÷ TPI) |
A | Tool angle, no decimal point (e.g. A60) |
P | Cutting method P1–P4 |
I | Taper (radius) |
G76 example program
(1"-16 UN external, lead 0.0625)
G97 S800 M03
G00 X1.1 Z0.25
G76 X0.9234 Z-1. K0.0383 D0.0115 F0.0625 A60 P2
G00 X3.⚠ Watch out
Start the tool at least three or four leads before the part so the spindle and axis can synchronise. Starting at Z0 cuts the first threads short and off-pitch. Use G97 (constant RPM), never G96, for threading.
Related codes
G76 questions
What is K in a Haas G76?
The full thread height measured per side (radius), not on diameter.
Should I thread in G96 or G97?
G97. Constant RPM keeps every pass in sync with the spindle.
Independent reference. Not affiliated with, sponsored by or endorsed by Haas Automation, Inc. Haas is a trademark of its respective owner. Always confirm codes against your machine's operator manual — options and settings vary by model and software version.