TAHA Engineering Toolsby TAHA Knowledge Lab

Machining & Workshop

Tap Drill Size Calculator

Tap drill diameter for ISO metric and UNC/UNF threads at your chosen % of thread.

Inputs

Cross-section of a threaded hole showing the major diameter D, the minor diameter D1 and the drilled hole diameter.DD₁drilled hole
Section through a tapped hole. The drill (dashed) is a little larger than the basic minor diameter D₁, so the tap cuts only part of the full thread depth — the “percentage of thread”. D is the nominal (major) diameter. Diagram not to scale.

75% is a common choice for cutting taps in steel. Higher percentages give little extra strength but make tapping harder and taps more likely to break. Lower values (60–70%) are often used in hard or tough materials. Above about 83% the drill is smaller than the basic minor diameter.

Result

Tap drill diameter (calculated)
5.02572
Rounded to nearest 0.1 mm
5 mm (≈ 77% thread)
Nearest fractional drill (1/64 in steps)
13/64 in (0.20313 in)
Basic minor diameter of the nut thread (100%)
4.91747
Thread percentage with the “D − P” rule
76.98%
Working
M6 × 1 (coarse): D = 6 mm, P = 1 mm Drill = D − 1.299 × P × %thread = 6 − 1.299 × 1 × 0.75 = 5.0257 mm

For 75% thread, drill 5.02572 mm (5 mm (≈ 77% thread)). Never drill smaller than the minor diameter, 4.91747 mm.

Educational estimate — check the assumptions below.

About this calculator

Before an internal thread is cut with a tap, a hole is drilled slightly larger than the inside (minor) diameter of the thread. The drill size controls the percentage of thread: how much of the full thread depth the tap cuts. A smaller drill gives more thread engagement but much higher tapping torque and a greater risk of breaking the tap. Around 75% is a common compromise: machining handbooks note that going much higher adds little strength but greatly increases tapping torque.

Choose a standard ISO metric or UNC/UNF size, or enter any 60° thread by diameter and pitch. For metric threads the familiar shop rule drill = D − P (for example M6 → 5 mm) gives about 77% thread.

Formula

ddrill = D − 1.299 × P × (%thread ÷ 100)

D1 = D − 1.0825 × P

D = nominal major diameter, P = pitch (for TPI: P = 25.4 mm ÷ TPI), D1 = basic minor diameter of the internal thread. In this widely used shop formula, “100% thread” means a thread depth of 0.6495 × P on each side (three-quarters of the 60° triangle height H), so 1.299 × P on the diameter. The basic minor diameter D1 corresponds to about 83%. Imperial form: drill (in) = D − 0.01299 × %thread ÷ TPI.

Worked example

  • M6 × 1, 75% thread: 6 − 1.299 × 1 × 0.75 = 5.03 mm → use a 5.0 mm drill (about 77% thread).
  • 1/4-20 UNC, 75%: 0.25 − 0.01299 × 75 ÷ 20 = 0.2013 in, which matches the common #7 drill (0.201 in).
  • M10 × 1.5: basic minor diameter = 10 − 1.0825 × 1.5 = 8.376 mm; an 8.5 mm drill gives about 77% thread.

Assumptions and limitations

  • For <strong>cutting</strong> taps in 60° threads (ISO metric and Unified). <strong>Forming (roll) taps</strong> need a larger hole — use the tap manufacturer’s recommended size.
  • The result is a theoretical drill diameter. Drills often cut slightly oversize; use the nearest available drill and check it does not give more than 100% thread.
  • Thread classes and tolerances (ISO 965, ASME B1.1) set minimum and maximum minor diameters for each thread. Where a drawing or standard specifies the minor diameter, that takes priority over this calculation.
  • Only major diameter and pitch of the listed standard sizes are used; no tolerance tables are included. Number-size drills (#1–#80) and letter drills are not listed.

References

  • ISO 68-1 and ASME B1.1 basic 60° thread profile (H = 0.866 P; basic minor diameter D − 1.0825 P).
  • ISO 261 / ISO 262 (metric sizes and pitches); ASME B1.1 (UNC/UNF sizes).
  • Percentage-of-thread relation: % = TPI × (D − drill) ÷ 0.01299 (standard machining texts).