M5x0.8 tap speeds and feeds

    A M5x0.8 tap feeds one pitch per turn: 0.8 mm per rev. With a general-purpose HSS tap, start near 1,360 RPM and 1,088 mm/min in 6061 aluminum, or 390 RPM and 312 mm/min in mild steel.

    ISO metric coarse thread · major Ø 5.00 mm · tap drill 4.2mm (4.20 mm) for a cut tap, 4.65 mm for a form tap.

    M5x0.8 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.

    M5x0.8 cut and form tap speeds
    MaterialCut SFMCut RPMCut mm/minForm SFMForm RPMForm mm/min
    Aluminum 6061 / 707570–901,360–1,7501,088–1,40065–1151,260–2,2301,008–1,784
    Free-machining / mild steel (12L14, 1018)20–40390–780312–62450–115970–2,230776–1,784
    4140 alloy steel (annealed to <35 HRC)20–30390–580312–46450–85970–1,650776–1,320
    304 / 316 stainless10–20190–390152–31215–40290–780232–624
    Tool steel (A2, D2, O1, H13, P20)15–25290–490232–3928–25160–490128–392
    Gray / ductile cast iron15–30290–580232–464Not listedNot listedNot listed
    Brass / bronze60–1001,160–1,940928–1,552Not listedNot listedNot listed
    Titanium (6Al-4V, CP)5–15100–29080–2328–15160–290128–232
    Plastics and composites (acetal, nylon, G-10)50–70970–1,360776–1,088Not 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.

    M5x0.8 premium cut tap speeds (OSG)
    MaterialOSG rowSFMRPMmm/min
    Aluminum 6061 / 7075Aluminum alloys70–1201,360–2,3301,088–1,864
    Free-machining / mild steel (12L14, 1018)Carbon steels <35 HRC80–1201,550–2,3301,240–1,864
    4140 alloy steel (annealed to <35 HRC)Alloy steels <35 HRC35–65680–1,260544–1,008
    304 / 316 stainlessStainless 300 & 400 series <35 HRC15–75290–1,460232–1,168
    Tool steel (A2, D2, O1, H13, P20)Alloy, tool & die steels 30–40 HRC15–30290–580232–464
    Gray / ductile cast ironCast iron50–120970–2,330776–1,864
    Titanium (6Al-4V, CP)Titanium alloys <35 HRC15–20290–390232–312

    Worked example: M5x0.8 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 ÷ 0.20 ≈ 1,360 RPM (D = 5 mm = 0.20 in; or RPM = 1000 × 21.3 m/min ÷ (π × 5)).
    3. Feed per rev = pitch = 0.8 mm.
    4. Feed = RPM × pitch = 1,360 × 0.8 = 1,088 mm/min (42.8 IPM).

    G84 tapping code for M5x0.8

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

    Fanuc rigid tap (M29)

    (M5x0.8 TAP - RIGID)
G21 G17 G40 G80 G90
T5 M06
G54 G00 X0. Y0.
G43 H05 Z25. M08
M29 S1360           (RIGID TAP MODE; M-CODE SET BY PARAMETER)
G98 G84 Z-8. R3. F1088.
G80 M09
G91 G28 Z0.
M30

    Haas rigid tap

    G21 G00 G90 G54 X0. Y0.
G43 H05 Z3. M08
G84 Z-8. R3. F1088. S1360   (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 S1360) and the same F1088 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 M5x0.8-LH taps use G74 instead of G84.
    • If the control caps rigid-tap RPM, lower S and recompute F: F = S × 0.8.

    Notes for this size

    • M5x0.8 is in the size range most shops rigid tap every day. Run the low end of the table first, then raise speed in 10% steps while watching spindle load on the reversal.
    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 M5x0.8

    Tap calculator, prefilled for M5x0.8M5x0.8 tap drill sizeTap drill chart

    Common questions

    What RPM for a M5x0.8 tap?
    RPM = 3.82 × SFM ÷ D with D = 0.20 in. With a general-purpose HSS tap that is about 1,360 RPM in 6061 aluminum (70 SFM) and 390 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 M5x0.8 tap?
    Feed per revolution equals the pitch: 0.8 mm. Feed (mm/min) = RPM × 0.8, so at 1,360 RPM the feed is 1,088 mm/min.
    How fast can I run a M5x0.8 form (roll) tap?
    OSG lists 65–115 SFM for form taps in aluminum alloys, which is 1,260–2,230 RPM for M5x0.8. Form taps need a larger hole: about 4.65 mm (4.65 mm).
    What speed for a M5x0.8 tap in stainless steel?
    General-purpose HSS taps: 10–20 SFM, or 190–390 RPM at 152–312 mm/min. 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 M5x0.8 (D = 5 mm). 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