Choosing the wrong tap drill size is one of the most common causes of broken taps and stripped threads. Drill too small and the tap binds and breaks. Drill too large and threads strip under load. This guide explains how tap drill sizes are calculated, how to look them up for UNC, UNF, and Metric threads, and when to deviate from the standard 75% thread engagement rule.
The tap drill diameter is calculated to leave approximately 75% thread engagement after tapping. Formula for Unified threads (UNC/UNF): Tap Drill ≈ Nominal diameter − (1 / TPI). Example: 1/4-20 UNC. Tap drill = 0.250 − (1/20) = 0.250 − 0.050 = 0.200". The standard tap drill is #7 (0.201"). For Metric threads: Tap drill = Nominal diameter − Pitch. Example: M8×1.25. Tap drill = 8 − 1.25 = 6.75 mm. This formula gives the theoretical diameter. Standard tables round to the nearest available drill size.
Standard 75% thread engagement works well for steel and most metals. However, the optimal engagement level depends on material strength. Strong materials (alloy steel, stainless, titanium): 60–70% engagement is sufficient and reduces tap load. Drilling slightly larger saves taps without losing meaningful strength. Soft materials (aluminum, plastic, magnesium): 75–85% engagement recommended because the material itself has lower shear strength. The thread, not the bolt, often fails first. Very soft materials (cast aluminum, low-density plastic): Consider thread inserts (Helicoil, Keensert) rather than relying on cut threads.
Thread size and standard drill: #6-32 UNC → #36 (0.1065"). #8-32 UNC → #29 (0.136"). #10-24 UNC → #25 (0.1495"). 1/4-20 UNC → #7 (0.201"). 5/16-18 UNC → F (0.257"). 3/8-16 UNC → 5/16" (0.3125"). 7/16-14 UNC → U (0.368"). 1/2-13 UNC → 27/64" (0.4219"). 5/8-11 UNC → 17/32" (0.5312"). 3/4-10 UNC → 21/32" (0.6562"). These are for 75% thread engagement in standard materials. UNF (fine pitch) drill sizes are slightly larger than UNC for the same nominal diameter — fine threads have a higher root minor diameter.
M3×0.5 → 2.5 mm. M4×0.7 → 3.3 mm. M5×0.8 → 4.2 mm. M6×1.0 → 5.0 mm. M8×1.25 → 6.75 mm (use 6.8 mm). M10×1.5 → 8.5 mm. M12×1.75 → 10.25 mm (use 10.2 mm). M14×2.0 → 12.0 mm. M16×2.0 → 14.0 mm. M20×2.5 → 17.5 mm. Metric tap drill calculation is simpler than Unified: always subtract the pitch from the nominal diameter. Standard metric taps are coarse pitch (ISO 261). Fine-pitch variants (M8×1.0, etc.) use a different drill size — always verify pitch before drilling.
1) Use a spotting drill (not a center drill) to start the hole accurately. Center drills deflect on flat surfaces. 2) Drill at the correct speed — see cutting speed calculator for your material. Drilling too fast in stainless work-hardens the surface. 3) Drill through-holes 0.1–0.2" deeper than the required thread depth to provide chip clearance for the tap. 4) Use cutting fluid appropriate to the material. Aluminum: WD-40 or aluminum cutting fluid. Steel: cutting oil or sulphurized fluid. Stainless: cutting oil — stainless work-hardens rapidly without lubricant. 5) For blind holes, use a plug tap first then a bottoming tap to cut threads to full depth.
Using a too-small tap drill increases thread engagement above 75%. This dramatically increases the torque required to cut the thread. The tap is more likely to break, especially in tough materials like stainless steel or alloy steel. Studies show that increasing thread engagement from 75% to 100% only adds about 5% to thread shear strength — but doubles or triples the tap breakage risk. Always use the standard tap drill size unless you have a specific engineering reason to deviate.
Yes, you can substitute a metric drill that is close in size to the standard drill. The key is to stay within about ±0.005" of the recommended tap drill diameter. Example: For a 1/4-20 UNC thread, the standard drill is #7 (0.201"). A 5.1 mm drill (0.2008") is an acceptable substitute. A 5.0 mm drill (0.197") is slightly under but workable for most materials. Always verify the substitution will give acceptable thread engagement for your application.
A tap drill creates the hole that will be tapped (threaded). It is undersized relative to the bolt to allow thread engagement. A clearance drill creates a hole that a bolt passes through freely without threading. Clearance holes are larger than the bolt's nominal diameter. For a 1/4-20 bolt: tap drill is #7 (0.201"), close clearance drill is 9/32" (0.281"), free clearance drill is 5/16" (0.313"). Never tap a clearance hole — the drill is too large.