About Tap Drill Size Calculator — Metric & UNC/UNF Threads
The tap drill size calculator finds the hole to drill before tapping an internal thread. Enter the thread — major diameter and pitch for ISO metric, major diameter and threads per inch for unified UNC/UNF — pick the percentage of full thread engagement you want (75% is the machine-shop default), and the tool applies the Machinery's Handbook formula: drill = major − 1.29904 × pitch × (% ÷ 100). It reports the theoretical drill diameter, the nearest standard drill from the metric or fractional/number/letter tables, and the thread engagement that standard drill actually gives.
More thread engagement is not better past a point: tests reported in Machinery's Handbook show engagement above about 75% adds little strength while making the tap dramatically harder to drive and easier to break, which is why published tap-drill charts are built on 75%. The classic shop rule for metric threads — tap drill = major minus pitch, e.g. 8.5 mm for M10×1.5 — is this same formula at exactly 76.98% engagement.
How It Works
- Pick the thread system. Metric threads take the basic major diameter in millimetres and the thread pitch in millimetres (an M10×1.5 thread is major 10, pitch 1.5). Unified threads take the major diameter in inches and threads per inch (a 1/4-20 UNC thread is major 0.25, TPI 20). Toggling systems converts your entries and clamps them to the valid range.
- Set the desired thread engagement between 50% and 85%. 75% is the default that published tap-drill charts assume; drop toward 60–65% for hard materials or deep holes where tap breakage is the risk, and only push above 75% for very shallow thread depths in soft material.
- Read the theoretical drill diameter from the formula drill = major − 1.29904 × pitch × %/100 (for inch threads pitch = 1/TPI, giving the handbook's drill = major − 0.01299 × %/TPI form).
- Use the nearest standard drill: the calculator searches the metric table (0.1 mm steps to 13 mm, 0.5 mm steps to 25 mm) for metric threads, or the combined fractional (1/64″ steps), number (#80–#1) and letter (A–Z) gauge tables for inch threads, and shows the engagement that drill actually produces so you can see how far it lands from your target.
- Check the cross-system substitute when the right drill is missing from your index — a 10.8 mm drill is often closer to the 1/2-13 theoretical size than any inch drill in the box.
Worked Example
Tap an M10×1.5 hole at the standard 75% thread engagement. The theoretical drill is 10 − 1.29904 × 1.5 × 0.75 = 10 − 1.461 = 8.539 mm. The nearest standard metric drill is 8.5 mm, and plugging 8.5 mm back through the formula gives (10 − 8.5) × 76.98 ÷ 1.5 = 76.98% engagement — the tap drill charts' familiar "major minus pitch" answer, slightly tighter than the 75% target but well inside the safe range. For the inch example, a 1/4-20 UNC thread at 75% needs 0.25 − 0.01299 × 75 ÷ 20 = 0.2013 in, and the nearest standard drill is the #7 gauge drill at 0.2010 in (75.4% actual engagement) — exactly what the printed charts list for 1/4-20.
Formulas
- Tap drill diameter (percentage of full thread)
drill = major − 1.29904 × p × (%TE / 100)- Handbook printed forms (same identity)
inch: drill = major − 0.01299 × %TE / TPI; metric: drill = major − p × %TE / 76.98- Engagement a given drill produces
%TE = (major − drill) × 100 / (1.29904 × p)
Standards & References
- Machinery's Handbook, Tapping and Thread Cutting — percentage-of-full-thread tap drill formulas (drill = major − 0.01299 × %/TPI; metric drill = major − pitch × %/76.98) and the guidance that engagement above ~75% adds little strength but raises tap-breakage risk
- ANSI/ASME B94.11M — twist drill standard defining the number (#80–#1) and letter (A–Z) gauge drill sizes used in the nearest-drill lookup
- ISO 68-1 / ASME B1.1 — 60° thread form the engagement factor 1.29904 = (3/4)√3 derives from
Frequently Asked Questions
What size drill bit do I use for an M10×1.5 tap?
Use an 8.5 mm drill for a standard 75% thread. The formula gives a theoretical 8.539 mm at exactly 75% engagement; 8.5 mm is the nearest standard drill and works out to 76.98% engagement — which is precisely why the shop rule "metric tap drill = major diameter minus pitch" (10 − 1.5 = 8.5) works for every ISO metric coarse and fine thread.
What is percentage of thread engagement and why is 75% the default?
It is how much of the full theoretical thread height the tapped thread actually engages. Tests reported in Machinery's Handbook show that going above about 75% engagement adds very little joint strength while the torque to drive the tap rises steeply — a 100% thread is only marginally stronger but several times harder to tap and far more likely to snap the tap in the hole. Published tap-drill charts therefore standardize on 75%.
When should I use less than 75% thread engagement?
Drop toward 60–65% for hard or gummy materials (stainless, tool steel, titanium), small taps that break easily, and deep holes where chip packing multiplies torque. The strength loss is small as long as the thread depth (length of engagement) is at least the nominal diameter — add engagement length, not thread percentage, when you need a stronger joint in soft material.
What drill do I use for a 1/4-20 tap?
A #7 number drill (0.2010 in). The 75% theoretical size is 0.25 − 0.01299 × 75 ÷ 20 = 0.2013 in, and #7 is the nearest standard drill at 75.4% actual engagement. The calculator also shows the closest metric substitute (5.1 mm = 0.2008 in) for when the number drill is missing from your index.
Why does the calculator clamp engagement to 50–85%?
Below about 50% the threads get so shallow that a fastener can strip under ordinary preload, and above about 85% the tapping torque and breakage risk climb out of proportion to any strength gain — Machinery's Handbook flags the region above ~75–80% as rarely justified. If you enter a value outside 50–85% the tool clamps it to the nearest bound and tells you, rather than silently computing a size you should not use.
Do these formulas work for cut taps and form (roll) taps alike?
They are for cut taps, which remove material. Form taps displace material instead, so the hole must start larger — form-tap drill sizes run roughly halfway between the cut-tap drill and the major diameter, and the manufacturer's recommended drill size for the specific tap should always win. The same 75%-engagement logic applies, but with the tap maker's own formula.