Why 'diameter minus pitch' actually works
Every machinist knows the shortcut. Fewer know it is the formula in disguise, or where it stops being safe to use.
5 min read
Why does diameter minus pitch give the right tap drill?
Because it is the full formula evaluated at about 77% thread engagement, which happens to be the shop standard. The formula is drill = diameter − (engagement ÷ 100) × 1.299 × pitch. At 77%, 0.77 × 1.299 comes to almost exactly 1.0, so the expression collapses to diameter minus pitch. For M8 × 1.25 that gives 6.75 mm against the chart value of 6.8 mm — a difference well inside normal drill tolerance.
Two constants, and the one people mix up
This is the error worth guarding against, because both numbers are correct for different things.
The minor diameter of an internal thread is diameter − 1.0825 × pitch. That is a real geometric quantity derived from the 60° thread form.
The tap drill for a given percentage of thread is diameter − (percentage ÷ 100) × 1.299 × pitch. Percent-of-thread is conventionally reckoned against a different reference height, which is why the constant differs.
Using 1.0825 in the tap drill formula puts every result about 3% of a diameter oversize. On M8 it gives 6.99 mm where every published chart says 6.8 mm.
The check is easy: if your formula does not reproduce 6.8 mm for M8 × 1.25 at 75%, you have the wrong constant.
Why 75% is the standard and not 100%
Thread strength does not scale with engagement in the way intuition suggests.
Going from 60% to 75% engagement adds meaningful strength. Going from 75% to 100% adds roughly 5% — while approximately tripling the torque required to cut the thread.
Since a tap fails in torsion, that is a badly one-sided trade. The extra torque is precisely what snaps a tap off flush with the surface of a blind hole in stainless, converting a two-minute operation into an afternoon with a carbide burr.
In practice the fastener fails before a 75% thread does, so the additional engagement buys nothing you can use.
75% is not a compromise. It is close to optimal for almost every real case.
When the shortcut stops being safe
The rule works because it lands near 75%. Outside that, it does not apply.
If you are deliberately cutting a lower engagement — common in hard or tough material where tapping torque is the binding constraint — work the formula properly. The same applies to a higher engagement in soft material.
The shortcut is also metric-specific in its familiar form, because metric threads state a pitch directly. For inch threads you must convert first: pitch in millimetres is 25.4 divided by threads per inch. A 1/4-20 UNC has a 1.27 mm pitch, and the formula returns 0.2013 in — the #7 drill every chart lists.
Where the shortcut applies it is excellent. Where it does not, it is silently wrong.
Do not forget the clearance hole
The tapped hole gets the attention; the hole the bolt passes through often does not, and drilling it at nominal diameter is a mistake.
An M8 bolt through an 8 mm hole binds on any misalignment at all. ISO 273 defines three fits — close, medium and free — and medium is the sensible default for general work, giving 9 mm for M8.
That extra millimetre is what allows two parts to actually come together. Use close only where location genuinely matters, and free where thermal movement or tolerance stack-up is in play.
A well-tapped hole and a too-tight clearance hole still make an assembly that will not go together.