1"-8 tap speeds and feeds

    A 1"-8 tap feeds one pitch per turn: 0.1250 in (1 ÷ 8 TPI) per rev. With a general-purpose HSS tap, start near 270 RPM and 33.8 IPM in 6061 aluminum, or 80 RPM and 10.0 IPM in mild steel.

    UNC thread · major Ø 1.0000 in · tap drill 7/8" (0.8750 in) for a cut tap, 15/16 for a form tap.

    1"-8 tapping speeds by material

    Cut tap = general-purpose HSS tap. Form tap = OSG form (roll) taps. RPM rounded to 10; IPM = RPM ÷ 8. Start at the low end.

    1"-8 cut and form tap speeds
    MaterialCut SFMCut RPMCut IPMForm SFMForm RPMForm IPM
    Aluminum 6061 / 707570–90270–34033.8–42.565–115250–44031.3–55.0
    Free-machining / mild steel (12L14, 1018)20–4080–15010.0–18.850–115190–44023.8–55.0
    4140 alloy steel (annealed to <35 HRC)20–3080–11010.0–13.850–85190–32023.8–40.0
    304 / 316 stainless10–2040–805.00–10.015–4060–1507.50–18.8
    Tool steel (A2, D2, O1, H13, P20)15–2560–1007.50–12.58–2530–1003.75–12.5
    Gray / ductile cast iron15–3060–1107.50–13.8Not listedNot listedNot listed
    Brass / bronze60–100230–38028.8–47.5Not listedNot listedNot listed
    Titanium (6Al-4V, CP)5–1520–602.50–7.508–1530–603.75–7.50
    Plastics and composites (acetal, nylon, G-10)50–70190–27023.8–33.8Not listedNot listedNot listed

    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.

    1"-8 premium cut tap speeds (OSG)
    MaterialOSG rowSFMRPMIPM
    Aluminum 6061 / 7075Aluminum alloys70–120270–46033.8–57.5
    Free-machining / mild steel (12L14, 1018)Carbon steels <35 HRC80–120310–46038.8–57.5
    4140 alloy steel (annealed to <35 HRC)Alloy steels <35 HRC35–65130–25016.3–31.3
    304 / 316 stainlessStainless 300 & 400 series <35 HRC15–7560–2907.50–36.3
    Tool steel (A2, D2, O1, H13, P20)Alloy, tool & die steels 30–40 HRC15–3060–1107.50–13.8
    Gray / ductile cast ironCast iron50–120190–46023.8–57.5
    Titanium (6Al-4V, CP)Titanium alloys <35 HRC15–2060–807.50–10.0

    Worked example: 1"-8 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 ÷ 1.0000 ≈ 270 RPM.
    3. Feed per rev = pitch = 0.1250 in (1 ÷ 8 TPI).
    4. IPM = RPM ÷ TPI = 270 ÷ 8 = 33.8 IPM.

    G84 tapping code for 1"-8

    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"-8 TAP - RIGID)
G20 G17 G40 G80 G90
T5 M06
G54 G00 X0. Y0.
G43 H05 Z1.0 M08
M29 S270           (RIGID TAP MODE; M-CODE SET BY PARAMETER)
G98 G84 Z-1.50 R0.1 F33.75
G80 M09
G91 G28 Z0.
M30

    Haas rigid tap

    G20 G00 G90 G54 X0. Y0.
G43 H05 Z0.1 M08
G84 Z-1.50 R0.1 F33.75 S270   (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 S270) and the same F33.75 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"-8-LH taps use G74 instead of G84.
    • If the control caps rigid-tap RPM, lower S and recompute F: F = S ÷ 8.

    Notes for this size

    • 1"-8 needs real torque: check that your spindle makes enough torque at 80 RPM (a gear-range spindle may need its low range). Thread milling is often the safer choice in tough material at this size.
    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.

    Hole and tools for 1"-8

    Tap calculator, prefilled for 1"-81"-8 tap drill sizeTap drill chart

    Common questions

    What RPM for a 1"-8 tap?
    RPM = 3.82 × SFM ÷ D with D = 1.0000 in. With a general-purpose HSS tap that is about 270 RPM in 6061 aluminum (70 SFM) and 80 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"-8 tap?
    Feed per revolution equals the pitch: 0.1250 in (1 ÷ 8 TPI). IPM = RPM ÷ 8, so at 270 RPM the feed is 33.8 IPM.
    How fast can I run a 1"-8 form (roll) tap?
    OSG lists 65–115 SFM for form taps in aluminum alloys, which is 250–440 RPM for 1"-8. Form taps need a larger hole: about 15/16 (0.9375 in).
    What speed for a 1"-8 tap in stainless steel?
    General-purpose HSS taps: 10–20 SFM, or 40–80 RPM at 5.00–10.0 IPM. Keep the tap cutting and use 60–65% thread to cut torque.

    Nearby sizes

    Sources

    SFM ranges are copied from the tables above; RPM and feed are computed for 1"-8 (D = 1.0000 in). Speeds are starting values: your tap maker's data, coolant and machine come first.

    Free for machinists & programmers

    Put your skills on a free talent profile

    Machines, controls, certs and saved calculations in one profile shops can find.

    Create free profile
    For your shop

    Bring shift handoffs to your shop

    Stop losing job status between shifts. Every station's notes, counts and issues, handed off cleanly.

    See shift handoffs