Haas Mill · G-code
G84 Tapping Canned Cycle
Rigid taps a right-hand thread: feeds in synchronised with the spindle, reverses, and feeds out.
What G84 does on a Haas mill
G84 feeds the tap to Z in sync with spindle rotation, reverses the spindle and feeds back out. The spindle must be running forward (M03) when the cycle starts. G74 is the left-hand version and needs M04.
In feed-per-minute mode (G94) F must equal RPM ÷ threads per inch (or RPM × pitch in metric). In feed-per-rev mode (G95) F is simply the pitch. Haas also offers a J retract multiplier to back out faster than you went in.
G84 format
| Address | Meaning |
|---|---|
X Y | Hole position |
Z | Depth |
R | R plane |
F | RPM ÷ TPI in G94, or the pitch in G95 |
J | Optional retract speed multiplier |
G84 example program
(1/4-20 tap at 500 RPM: F = 500 / 20 = 25.)
S500 M03
G84 G99 X1. Y1. Z-0.5 R0.2 F25.
X2.
G80⚠ Watch out
Change the RPM and forget to recalculate F and the tap is either stretched or crushed. Using G95 with F = pitch removes that mistake entirely.
Related codes
G84 questions
How do I calculate feed for G84 on a Haas?
F = RPM ÷ TPI in inch G94 mode. For a 1/4-20 at 500 RPM, F25. In G95, F is the pitch: 0.05 for 20 TPI.
Does G84 need M03?
Yes. G84 is right-hand and expects the spindle running forward; G74 is left-hand with M04.
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.