Skip to content
MachineCalcs

Tap Drill Size Calculator

Tap drill diameter for any standard metric or unified thread at your chosen % thread engagement, with the major diameter, pitch and 100% minor diameter. Metric and imperial.

Inputs

Results

Tap drill diameter
5.026 mm

M6 at 75% thread.

Use the nearest available drill.

Major diameter
6 mm

Thread pitch
1 mm

Minor diameter (100%)
4.918 mm

Basic internal minor, d − 1.0825·pitch.

  • % thread is the chart convention: % = 76.98 × (major − tap drill) ÷ pitch. The "major − pitch" rule of thumb gives ≈ 77%.
  • Use the nearest standard drill at or just above this size; going under raises tapping torque and tap breakage sharply for little extra strength.
  • 50–65% thread is plenty in most materials and far easier to tap; reserve 75%+ for thin or soft sections.

How it works

The tap drill leaves enough material for the tap to cut threads to a chosen depth — the percent of thread engagement. The drill diameter is: tap drill = major − (%thread × pitch) / 76.98 The constant 76.98 comes from the 60° thread geometry, and it is the convention printed on tap-drill charts. The familiar shortcut “tap drill = major − pitch” is just this formula at about 77% thread.

Higher engagement is not better: most of a thread’s strength is in the first few threads, so going from 65% to 75% roughly doubles the tapping torque for a negligible strength gain. For hard materials, deep holes or small taps, 50–65% engagement taps far more safely.

Worked example

An M6 thread has a 1 mm pitch. At 75% engagement the tap drill is 6 − (75 × 1) / 76.98 ≈ 5.03 mm, so you would use a 5.0 mm drill — the classic M6 tap drill. The basic minor diameter is 6 − 1.0825 × 1 ≈ 4.92 mm. The calculator returns these directly.

Reference data

Standard threads with their major diameter, pitch and the tap drill at 75% engagement.

Tap drill sizes at 75% thread engagement.
Thread Major Ø (mm) Pitch (mm) Tap drill @75% (mm)
M3 3 0.5 2.51
M4 4 0.7 3.32
M5 5 0.8 4.22
M6 6 1 5.03
M8 8 1.25 6.78
M10 10 1.5 8.54
M12 12 1.75 10.3
M16 16 2 14.1
M20 20 2.5 17.6
M24 24 3 21.1
M8x1 8 1 7.03
M10x1.25 10 1.25 8.78
M12x1.25 12 1.25 10.8
1/4-20 UNC 6.35 1.27 5.11
5/16-18 UNC 7.9375 1.4111 6.56
3/8-16 UNC 9.525 1.5875 7.98
1/2-13 UNC 12.7 1.9538 10.8
1/4-28 UNF 6.35 0.9071 5.47
3/8-24 UNF 9.525 1.0583 8.49

Source: ISO 261/262 (metric) and ASME B1.1 (unified). Verify against a current tap-drill chart and your tap maker's recommendation.

Frequently asked questions

How do I calculate tap drill size?
Tap drill = major diameter − (%thread × pitch) ÷ 76.98 for 60° threads. For an M6 (1 mm pitch) at 75% thread that is 6 − 0.97 ≈ 5.0 mm.
What percentage of thread engagement should I use?
About 75% is the traditional default, but 60–65% is plenty for most jobs and taps far more easily, with very little loss of strength. Drop toward 50% in hard materials or deep holes.
Is 75% thread really necessary?
Rarely. Almost all of a thread’s strength is carried by the first few engaged threads, and going from 65% to 75% roughly doubles the tapping torque for only a few percent more strength. Higher % mainly raises tap-breakage risk.
What is the tap drill for M6, M8 and M10?
At about 75% thread: M6 → 5.0 mm, M8 → 6.8 mm, M10 → 8.5 mm. See the table for the full list and pick the nearest available drill.
What is the minor diameter?
The basic internal minor diameter is major − 1.0825 × pitch — the diameter at 100% thread form. Tap drills sit above it because real threads do not need to be cut to a perfect sharp root.
Does this cover metric and inch threads?
Yes — metric coarse and fine plus unified UNC/UNF. Toggle SI/Imperial to read the drill size in mm or inches.

Method & assumptions

  • 60° ISO/Unified threads; the % thread uses the chart convention (76.98 constant).
  • Cut taps — roll/form taps need a larger hole (no chips removed); follow the form-tap maker’s chart.
  • Round up to the nearest available drill; under-size holes raise torque and break taps.

Related calculators