M3.5x0.6 tap speeds and feeds

M3.5x0.6 tapping speeds by material

Cut tap = general-purpose HSS tap. Form tap = OSG form (roll) taps. RPM rounded to 10; feed in mm/min = RPM × pitch. 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: M3.5x0.6 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 ÷ 0.14 ≈ 1,940 RPM (D = 3.5 mm = 0.14 in; or RPM = 1000 × 21.3 m/min ÷ (π × 3.5)).
3. Feed per rev = pitch = 0.6 mm.
4. Feed = RPM × pitch = 1,940 × 0.6 = 1,164 mm/min (45.8 IPM).

G84 tapping code for M3.5x0.6

Rigid tapping, aluminum numbers from the example, metric (G21), depth 1.5 × D. Check your control's manual before running.

Fanuc rigid tap (M29)

(M3.5x0.6 TAP - RIGID)
G21 G17 G40 G80 G90
T5 M06
G54 G00 X0. Y0.
G43 H05 Z25. M08
M29 S1940           (RIGID TAP MODE; M-CODE SET BY PARAMETER)
G98 G84 Z-5. R3. F1164.
G80 M09
G91 G28 Z0.
M30

Haas rigid tap

G21 G00 G90 G54 X0. Y0.
G43 H05 Z3. M08
G84 Z-5. R3. F1164. S1940   (NO M03 NEEDED)
(PECK: ADD Q = PECK DEPTH; J2 = RETRACT 2X, SEE SETTING 130)
G80 G00 Z25. M09

Floating / tension-compression holder

Without rigid tapping, run G84 with the spindle on (M03 S1940) and the same F1164 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 M3.5x0.6-LH taps use G74 instead of G84.
• If the control caps rigid-tap RPM, lower S and recompute F: F = S × 0.6.

Notes for this size

• M3.5x0.6 is a small tap: breakage, not speed, is the limit. Use 60–65% thread, a spiral-point tap in through holes, and a holder with torque protection if you tap by hand-fed spindle.

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 M3.5x0.6 tap?

RPM = 3.82 × SFM ÷ D with D = 0.14 in. With a general-purpose HSS tap that is about 1,940 RPM in 6061 aluminum (70 SFM) and 550 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 M3.5x0.6 tap?

Feed per revolution equals the pitch: 0.6 mm. Feed (mm/min) = RPM × 0.6, so at 1,940 RPM the feed is 1,164 mm/min.

How fast can I run a M3.5x0.6 form (roll) tap?

OSG lists 65–115 SFM for form taps in aluminum alloys, which is 1,800–3,190 RPM for M3.5x0.6. Form taps need a larger hole: about 3.2 mm (3.20 mm).

What speed for a M3.5x0.6 tap in stainless steel?

General-purpose HSS taps: 10–20 SFM, or 280–550 RPM at 168–330 mm/min. Keep the tap cutting and use 60–65% thread to cut torque.

Nearby sizes