How tap drill sizing works
A tap cuts internal threads in a machined part. Before tapping, you drill a smaller hole — the tap drill. If the hole is too small, the tap removes too much metal, torque spikes, and breakage risk goes up. If it is too large, threads are shallow and weak. For cutting taps, this calculator uses standard 75% tap drill charts (shop reference tables). Forming taps still use the roll-tap formula below.
The math behind tap drill size
For straight 60° threads (UNC, UNF, and ISO metric), tap drill diameter depends on major diameter, pitch, and the thread height you want left in the part. These formulas follow Machinery's Handbook practice and match Machining Doctor and common shop charts.
Cutting tap · inch (UNC / UNF)
D = D_major − Hp / (76.98 × TPI)
Cutting tap · inch (pitch P)
D = D_major − (Hp × P) / 76.98
Cutting tap · metric
D = D_major − (Hp × P) / 76.98
Forming tap · inch (UNC / UNF)
D = D_major − Hp / (175 × TPI)
Forming tap · inch (pitch P)
D = D_major − (Hp × P) / 175
Forming tap · metric
D = D_major − (Hp × P) / 175
- D
- Tap drill diameter (pre-tap hole), in mm or inches.
- D_major
- Nominal major thread diameter (bolt/screw OD), same units as D.
- P
- Thread pitch: mm on metric threads, or P = 1 ÷ TPI on inch threads.
- TPI
- Threads per inch (UNC / UNF inch threads only).
- Hp
- Thread height as % of the full 60° profile; 75% is the usual shop value.
- 76.98
- Divisor for cutting taps (60° UN / ISO profile).
- 175
- Divisor for forming taps (roll tap).
NPT pipe threads are tapered — use pipe tap drill tables; the formulas above do not apply.
Cutting tap vs forming tap
The calculator lets you pick tap type. Drilling for a cutting tap is not the same as drilling for a forming tap that displaces metal instead of removing it:
- Cutting tap: removes chips; uses divisor 76.98 in the formulas above (smaller hole for the same Hp).
- Forming tap (roll tap): displaces metal without chips; uses divisor 175 in the same formulas (larger hole at the same Hp).
- Both methods use the same Hp target (default 75%); only the divisor changes.
- NPT pipe threads are tapered — use pipe tap drill tables; the straight-thread formulas do not apply.
Shop tip: In blind holes, hard materials, or form taps, a slightly larger drill lowers torque and extends tap life. Always verify against your drawing, thread class, and the tap you will actually run.
Picking the right standard drill
Your calculated tap drill will almost never match a stocked size exactly. Round up to the next number, letter, fractional, or metric drill (see the reference tables below). Rounding up cuts engagement by 1–3% — that is the safe shop practice. Rounding down overloads the tap.
Thread systems in the calculator
UNC (coarse) and UNF (fine) cover most inch fasteners — e.g. #0-80 is UNF only, not UNC. Metric Coarse and Metric Fine are the most common ISO threads on CNC parts. NPT is for tapered pipe connections — drill sizes come from pipe tables, not these formulas.