Calculate tapping RPM and feed rate from tap size, thread pitch (TPI or metric) and workpiece material, or enter your own cutting speed in SFM or m/min.

Material speeds are typical general-purpose tap values; use your tap maker’s figure when you have it.

Single-start threads: pitch equals advance per revolution.

Ideal travel time (optional)
Blank omits the time estimate; zero gives zero ideal travel. Equal feed in and out; no acceleration or reversal allowance.

Tapping Speed Formula

This calculator relates spindle RPM, cutting surface speed, and pitch-synchronized axial feed. For a single-start tap, the feed advances one thread pitch per spindle revolution. In rigid tapping, spindle rotation and axial feed must stay synchronized; cutting surface speed and axial feed are different quantities.

F = N × P

Where:

Symbol Meaning Typical Units
F Tapping feed rate mm/min, m/min, in/min, ft/min
N Spindle speed RPM or RPS
P Thread pitch or linear advance per revolution mm/rev or in/rev

If the thread is entered as threads per inch, convert it to pitch first.

Pin / rev = (1) / (TPI)
Pmm / rev = (25.4) / (TPI)

If your source data is threads per millimeter (TPMM), invert it to get mm/thread pitch before entering it. The calculator accepts threads/in or mm/thread; it does not have a TPMM input.

Pmm / rev = (1) / (TPMM)

Direct Equations Used by the Calculator

The calculator displays axial feed in mm/min and in/min and takes spindle speed in RPM. The equations below also show manual conversions to m/min, ft/min, RPS and TPMM; those are not additional input or output controls.

Fmm / min = RPM × Pmm / rev
Fm / min = (RPM × Pmm / rev) / (1000)
Fin / min = (RPM) / (TPI)
Fft / min = (RPM) / (12 × TPI)
RPM = 60 × RPS

If you know threads per millimeter instead of pitch, the metric feed equation can be written directly as:

Fm / min = (RPM) / (1000 × TPMM)

How to Calculate Tapping Feed Rate

  1. Select threads per inch (TPI) or metric pitch in mm/thread.
  2. In RPM to synchronized feed mode, enter spindle speed in RPM. Convert any RPS value by multiplying by 60 first.
  3. Convert the thread count to pitch if needed.
  4. Select Calculate to multiply spindle RPM by advance per revolution and obtain synchronized linear feed.
  5. Read both mm/min and in/min. Use the manual conversion equations if a different machine display requires m/min or ft/min.

This is especially important on CNC machines using rigid tapping, because the commanded feed must match thread lead. For standard single-start taps, lead and pitch are the same; multi-start threads require lead rather than single-start pitch. Optional depth gives ideal time = 2 × depth / feed for equal entry and withdrawal rates, without approach, chamfer, acceleration, dwell or reversal allowance. A blank depth omits time; zero depth gives zero ideal travel.

Rearranged Forms

The calculator can solve RPM from linear feed and pitch, or RPM from a recommended cutting surface speed and tap diameter. The further pitch, TPI and TPMM rearrangements below are useful for hand calculations; they are not extra solve modes.

N = (F) / (P)
P = (F) / (N)
TPI = (RPM) / (Fin / min)
TPI = (RPM) / (12 × Fft / min)
TPMM = (RPM) / (1000 × Fm / min)

Examples

A metric thread with a 1.25 mm pitch running at 500 RPM requires this feed:

Fmm / min = 500 × 1.25 = 625
Fm / min = (625) / (1000) = 0.625

An imperial thread of 20 TPI running at 300 RPM gives this feed:

Fin / min = (300) / (20) = 15
Fft / min = (15) / (12) = 1.25

Quick Reference at 500 RPM

Thread Pitch / Advance per Rev Feed Rate
8 TPI 0.125 in/rev 5.208 ft/min
10 TPI 0.100 in/rev 4.167 ft/min
13 TPI 0.0769 in/rev 3.205 ft/min
20 TPI 0.0500 in/rev 2.083 ft/min
0.80 mm pitch 0.80 mm/rev 0.400 m/min
1.00 mm pitch 1.00 mm/rev 0.500 m/min
1.25 mm pitch 1.25 mm/rev 0.625 m/min
1.50 mm pitch 1.50 mm/rev 0.750 m/min
2.00 mm pitch 2.00 mm/rev 1.000 m/min

Unit Conversions

1 m / min ≈ 3.28084 ft / min
1 ft / min = 0.3048 m / min

Important Notes for Machining

  • The calculator synchronizes feed and RPM and can convert a user-entered recommended cutting speed to RPM. It offers typical general-purpose tap speeds by material as an estimate; use your tap maker’s figure when you have one. The D − P drill estimate is only a rough cutting-tap rule, not a universal 75% engagement calculation or a forming-tap drill recommendation; use the tap maker’s chart.
  • Recommended RPM depends on workpiece material, tap diameter, tool coating, lubrication, hole depth, and machine rigidity.
  • If feed is too fast for the actual pitch, the tap can bind or break. If feed is too slow, the threads can tear, rub, or go out of form.
  • Rigid tapping requires the feed command to stay locked to spindle rotation. Floating holders can absorb some mismatch, but they do not replace correct feed calculation.
  • For blind holes, leave room for chip evacuation and reversal so the tap does not bottom out before the cycle ends.

Common Mistakes

  • Confusing TPI with pitch. TPI is a count, while pitch is the distance traveled in one revolution.
  • Mixing RPM and RPS without converting between them.
  • Treating tapping feed rate as the same thing as cutting surface speed.
  • Entering metric pitch values as threads per millimeter, or vice versa.
  • Using the right RPM but the wrong feed units when programming the machine.

FAQ

Is tapping speed the same as spindle speed?
No. Spindle speed is rotational motion, while tapping speed here is the axial feed rate created by that rotation and the thread pitch.
Why does feed have to match pitch exactly?
For a single-start tap, each revolution advances it by one pitch. Multi-start threads follow lead rather than single-start pitch. A mismatch forces the tool to pull or push against the thread form.
Can I use this for metric and imperial threads?
Yes. The calculator supports both systems as long as the thread input and output units are selected consistently.