1-1/2-12 tap speeds and feeds

1-1/2-12 tapping speeds by material

Cut tap = general-purpose HSS tap. Form tap = OSG form (roll) taps. RPM rounded to 10; IPM = RPM ÷ 12. Start at the low end.

Not listed = no form-tap value in the cited tables (OSG lists no form tap for cast iron; brass and plastics are not in its form-tap table).

Premium coated cut taps on a rigid CNC

OSG's starting speeds for its premium HSS-E cut taps (A-Tap family and the titanium/stainless taps it names) are higher than the general-purpose row. Use them only with that class of tap and rigid tapping.

Worked example: 1-1/2-12 in 6061 aluminum

1. Surface speed: 70 SFM (low end of 70–90 for a general-purpose HSS tap).
2. RPM = 3.82 × SFM ÷ D = 3.82 × 70 ÷ 1.5000 ≈ 180 RPM.
3. Feed per rev = pitch = 0.0833 in (1 ÷ 12 TPI).
4. IPM = RPM ÷ TPI = 180 ÷ 12 = 15.0 IPM.

G84 tapping code for 1-1/2-12

Rigid tapping, aluminum numbers from the example, inch (G20), depth 1.5 × D. Check your control's manual before running.

Fanuc rigid tap (M29)

(1-1/2-12 TAP - RIGID)
G20 G17 G40 G80 G90
T5 M06
G54 G00 X0. Y0.
G43 H05 Z1.0 M08
M29 S180           (RIGID TAP MODE; M-CODE SET BY PARAMETER)
G98 G84 Z-2.25 R0.1 F15.00
G80 M09
G91 G28 Z0.
M30

Haas rigid tap

G20 G00 G90 G54 X0. Y0.
G43 H05 Z0.1 M08
G84 Z-2.25 R0.1 F15.00 S180   (NO M03 NEEDED)
(PECK: ADD Q = PECK DEPTH; J2 = RETRACT 2X, SEE SETTING 130)
G80 G00 Z1. M09

Floating / tension-compression holder

Without rigid tapping, run G84 with the spindle on (M03 S180) and the same F15.00 feed, but hold the tap in a tension-compression holder: it absorbs the overrun when the spindle stops and reverses. Leave the holder room to float at the bottom, so program the depth a little short and follow the holder maker's setting.

• Peck tapping (Q) clears chips in deep or blind holes in stainless and 4140; skip it in aluminum unless chips pack.
• Left-hand 1-1/2-12-LH taps use G74 instead of G84.
• If the control caps rigid-tap RPM, lower S and recompute F: F = S ÷ 12.

Notes for this size

• 1-1/2-12 needs real torque: check that your spindle makes enough torque at 50 RPM (a gear-range spindle may need its low range). Thread milling is often the safer choice in tough material at this size.
• UNF has a finer pitch than UNC at the same diameter, so the feed per rev is smaller and the tap removes less per tooth, but a fine-pitch tap is more sensitive to the spindle and feed staying in sync.

4140 alloy steel (annealed to <35 HRC)

Prehardened 4140 (28–32 HRC) is at the top of this band: use the low end and 50–65% thread.

304 / 316 stainless

Work-hardens: never let the tap dwell or rub, and use a tap made for stainless. 60–65% thread cuts torque sharply.

Tool steel (A2, D2, O1, H13, P20)

Values are for annealed or prehardened stock. Tap before heat treat whenever you can; hardened tool steel needs a thread mill or a carbide tap.

Common questions

What RPM for a 1-1/2-12 tap?

RPM = 3.82 × SFM ÷ D with D = 1.5000 in. With a general-purpose HSS tap that is about 180 RPM in 6061 aluminum (70 SFM) and 50 RPM in mild steel (20 SFM). Premium coated taps on a rigid CNC can run faster; see the second table.

What is the feed rate for a 1-1/2-12 tap?

Feed per revolution equals the pitch: 0.0833 in (1 ÷ 12 TPI). IPM = RPM ÷ 12, so at 180 RPM the feed is 15.0 IPM.

How fast can I run a 1-1/2-12 form (roll) tap?

OSG lists 65–115 SFM for form taps in aluminum alloys, which is 170–290 RPM for 1-1/2-12. Form taps need a larger hole: about 1-15/32 (1.4688 in).

What speed for a 1-1/2-12 tap in stainless steel?

General-purpose HSS taps: 10–20 SFM, or 30–50 RPM at 2.50–4.17 IPM. Keep the tap cutting and use 60–65% thread to cut torque.

Nearby sizes