← AskMachinist · Guides · Calculator · 🔎 Search

Percent of Thread and Form Tap Drill Size

Guide · Updated October 28, 2026

Percent of thread describes how deep the internal thread is compared with a full, theoretical V-thread. It is set almost entirely by the tap drill: a smaller drill leaves more metal for the tap to cut and gives a higher percentage. The classic machinist formula from Machinery's Handbook and tap makers is % thread = TPI × (basic major diameter − drill diameter) ÷ 0.01299. The constant comes from 1.299 × pitch, the double height of 75% of a sharp V thread (0.866P × 0.75 × 2). Metric is the same idea with pitch P in mm: % thread = 76.98 × (D − drill) ÷ P, since 1 ÷ 1.299 = 0.7698.

Need an exact reference size?

Build any gage block stack with the free Gage Block Calculator. Free, no login.

Step by step

Get the thread data: Basic major diameter and TPI (or pitch in mm).
Pick a candidate drill: Start from the tap drill chart.
Calculate percent: % = TPI × (D − drill) ÷ 0.01299, or 76.98 × (D − drill) ÷ P for metric.
Compare with the target: About 75% for general work, 50–65% for tough or deep holes.
Adjust the drill: A larger drill lowers percentage and torque; a smaller one raises both.
Check the result: Use a thread plug gage; GO must enter, NO-GO must not.

Percent of thread for common tap drills

1/4-20, #7 drill (0.2010): 75% thread
1/4-20, 13/64 (0.2031): 72% thread
5/16-18, F (0.2570): 77% thread
3/8-16, 5/16 (0.3125): 77% thread
1/2-13, 27/64 (0.4219): 78% thread
10-32, #21 (0.1590): 76% thread
8-32, #29 (0.1360): 69% thread

These come straight from the formula and assume the drilled hole is exactly drill size. In practice drills cut slightly oversize, often 0.001–0.003 in, so actual thread percentage runs a little lower. Ream or measure with pin gages when it matters.

Why 75% is usually enough

Tests reported by tap makers and in Machinery's Handbook show that going from 75% to 100% thread adds only about 5% more strength but roughly triples the tapping torque. In tough material like stainless or titanium, or in holes deeper than about 1.5 × diameter, 60–65% is common because tap breakage risk falls quickly and the bolt is still stronger than the threads need. Thin sheet is the exception, where more percentage helps make up for short engagement.

Metric tap drills

M3 x 0.5: cut-tap drill 2.5 mm (D − P, about 77%); form-tap drill about 2.75 mm (D − 0.5 P)
M4 x 0.7: cut-tap drill 3.3 mm (D − P, about 77%); form-tap drill about 3.65 mm (D − 0.5 P)
M5 x 0.8: cut-tap drill 4.2 mm (D − P, about 77%); form-tap drill about 4.60 mm (D − 0.5 P)
M6 x 1: cut-tap drill 5.0 mm (D − P, about 77%); form-tap drill about 5.50 mm (D − 0.5 P)
M8 x 1.25: cut-tap drill 6.8 mm (D − P, about 77%); form-tap drill about 7.38 mm (D − 0.5 P)
M10 x 1.5: cut-tap drill 8.5 mm (D − P, about 77%); form-tap drill about 9.25 mm (D − 0.5 P)
M12 x 1.75: cut-tap drill 10.2 mm (D − P, about 77%); form-tap drill about 11.12 mm (D − 0.5 P)

The D − P rule gives about 77% thread and is the basis of most metric cut-tap charts. The form-tap values use D − 0.5P, a common starting point; final form-tap hole sizes should come from the tap maker's chart because forming moves metal up into the crest.

Roll-form tap drill formula (inch)

Form taps do not cut chips; they displace metal, so they need a larger hole. A common starting formula is drill = basic major diameter − (0.0068 × target % thread) ÷ TPI, usually for 60–65% thread.

1/4-20 at 65%: 0.2279 in
5/16-18 at 65%: 0.2879 in
3/8-16 at 65%: 0.3474 in
10-32 at 65%: 0.1762 in
1/2-13 at 65%: 0.4660 in

Round to the nearest available drill and confirm against the tap maker's recommended hole size, since form taps are sensitive to hole size and material ductility. Form tapping works in ductile metals such as aluminum, low-carbon steel, copper and many stainless grades, not in cast iron or brittle alloys.

Worked example: 1/4-20 in 304 stainless

The chart drill is #7 (0.2010) for about 75%. Calculation: 20 × (0.2500 − 0.2010) ÷ 0.01299 = 20 × 0.049 ÷ 0.01299 = 75.4%. In 304, you want less torque, so try 13/64 (0.2031): 20 × 0.0469 ÷ 0.01299 = 72.2%. Going to a #6 (0.2040) gives 20 × 0.046 ÷ 0.01299 = 70.8%. All still gage on a 2B plug gage if the drill cuts true, and the larger drill noticeably reduces tap load.

Worked example: M8 x 1.25 in aluminum

Cut tap: 8 − 1.25 = 6.75 mm, which gives 76.98 × 1.25 ÷ 1.25 = 77%. With a 6.8 mm drill: 76.98 × 1.20 ÷ 1.25 = 73.9%. Both are fine. For a form tap, start at 8 − 0.625 = 7.375 mm, so a 7.4 mm drill, and check the tap maker's chart.

Common problems

Using a cut-tap drill with a form tap (breaks taps), drilling undersize in stainless for "more thread" (also breaks taps), and forgetting that drills cut oversize. Measure the hole with pin gages, which you can check against gage blocks, if threads fail the gage.

FAQ

What is the formula for percent of thread?

% thread = TPI × (major diameter − drill) ÷ 0.01299 for inch threads.

What percent thread does a #7 drill give in 1/4-20?

About 75%.

Is 100% thread stronger?

Only about 5% stronger than 75%, with roughly three times the tapping torque.

What size drill for a 1/4-20 form tap?

About 0.228 in from the formula at 65%; confirm on the tap maker's chart.

What is the metric tap drill rule?

Major diameter minus pitch, for example M6 x 1 uses a 5.0 mm drill.

Related guides and calculators

Build your stack in seconds

The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.

Questions? Ask a machinist.

General shop information only — follow your drawing, tool maker's data and your quality system.