Tap drill chart and how to read thread sizes (UNC, UNF, M-series)

Tap drill = major diameter − (0.01299 × % engagement / TPI). For the most common case - 1/4-20 at 75% thread - that's 0.250 − (0.01299 × 75 / 20) = 0.2013", so you grab a #7 drill (0.201"). Pick the wrong tap drill and you either snap the tap, strip the threads, or end up with a hole that fights you for the rest of the job. The math is simple - and it's the same math whether you're cutting on a Bridgeport, a CNC, or a hand drill in the field.

The two formulas

Imperial:   tap drill (in) = major Ø − 0.01299 × (% thread) / TPI
Metric:     tap drill (mm) = major Ø − 0.01299 × (% thread) × pitch

major Ø   = nominal thread diameter
TPI       = threads per inch (UNC/UNF)
pitch     = mm per thread (M-series)
% thread  = whole number: 75 for general work, 60 for hard/tough alloys

Check: 1/4-20 at 75% → 0.250 − 0.01299 × 75 / 20 = 0.2013" → #7 (0.201")

That's it. Both formulas land on the same physics - you're just backing off from the major diameter by enough to leave the tap room to cut clean threads.

Which "full thread" does the percentage mean? The % in these formulas is measured against the theoretical sharp-V profile - the basis Machinery's Handbook and every published tap chart use. Some references instead measure against the flatted UN/ISO design form (100% = the basic minor diameter, major − 1.0825 × pitch), and the same drill computes to a different percentage. When two charts or forum posts disagree about what "75%" means, that's the whole argument. Use the sharp-V formula above and your numbers will match the charts on this page.

UNC tap drill chart (75% thread)

• #4-40 - drill #43 (0.0890")
• #6-32 - drill #36 (0.1065")
• #8-32 - drill #29 (0.1360")
• #10-24 - drill #25 (0.1495")
• 1/4-20 - drill #7 (0.2010")
• 5/16-18 - drill F (0.2570")
• 3/8-16 - drill 5/16" (0.3125")
• 1/2-13 - drill 27/64" (0.4219")
• 5/8-11 - drill 17/32" (0.5313")
• 3/4-10 - drill 21/32" (0.6563")

UNF tap drill chart (75% thread)

• #10-32 - drill #21 (0.1590")
• 1/4-28 - drill #3 (0.2130")
• 5/16-24 - drill I (0.2720")
• 3/8-24 - drill Q (0.3320")
• 1/2-20 - drill 29/64" (0.4531")
• 5/8-18 - drill 9/16" (0.5625")
• 3/4-16 - drill 11/16" (0.6875")

Metric tap drill chart (M-series, 75% thread, coarse)

• M3 × 0.5 - drill 2.5 mm
• M4 × 0.7 - drill 3.3 mm
• M5 × 0.8 - drill 4.2 mm
• M6 × 1.0 - drill 5.0 mm
• M8 × 1.25 - drill 6.8 mm
• M10 × 1.5 - drill 8.5 mm
• M12 × 1.75 - drill 10.2 mm
• M16 × 2.0 - drill 14.0 mm
• M20 × 2.5 - drill 17.5 mm

Metric: the subtract-the-pitch rule

For metric coarse threads you don't even need the chart - subtract the pitch from the major diameter. M6 × 1.0 → 5.0 mm. M8 × 1.25 → 6.75, so grab a 6.8 mm. M10 × 1.5 → 8.5 mm. That's the entire chart above, compressed into one rule you can do in your head at the drill index.

Why it works: run the real formula at 75% and you get major − 0.01299 × 75 × pitch = major − 0.974 × pitch. Subtracting the full pitch takes off only a hair more than the 75% math calls for - about 77% on paper. Keep it honest, though: the rule slightly overshoots the engagement target, and twist drills cut a touch oversize anyway, which is exactly why the finished hole lands right around 75% in practice. The rule and the chart aren't rivals - they're the same number rounded to the nearest stock drill.

Tap drill vs clearance drill

Two different holes that get mixed up constantly. A tap drill leaves material for the threads to bite into. A clearance drill is bigger than the bolt so it passes straight through - no threads at all. For a 1/4" bolt: close fit is an F drill (0.257"), free fit is H (0.266"). Tap the clearance hole and nothing grips; try to push a bolt through a tap drill hole and it won't fit.

Bolt       Tap drill (75% UNC)    Clearance close     Clearance free
1/4-20     #7      (0.201")       F      (0.257")     H      (0.266")
5/16-18    F       (0.257")       P      (0.323")     Q      (0.332")
3/8-16     5/16"   (0.3125")      W      (0.386")     X      (0.397")
1/2-13     27/64"  (0.4219")      33/64" (0.5156")    17/32" (0.5313")

NPT pipe taps

Pipe threads are their own animal: NPT is tapered (3/4" per foot), so the tap cuts progressively bigger threads as it goes deeper and the joint tightens as it wedges. The drill sizes are nothing like the straight-thread math above:

NPT size   Tap drill
1/8-27     R      (0.339")
1/4-18     7/16"  (0.4375")
3/8-18     37/64" (0.578")
1/2-14     23/32" (0.719")
3/4-14     59/64" (0.922")

A straight drill only roughs the bore - for pressure-tight work, follow it with a tapered pipe reamer before tapping so the tap cuts an even depth of thread top to bottom instead of full threads at the top and shallow ones at the bottom. Depth of tap engagement sets the fit, and NPT still needs thread sealant (PTFE tape or pipe dope) to seal - only NPTF Dryseal is designed to seal dry.

Number and letter drills decoded

Wire-gauge (number) drills run from #80 (0.0135") up to #1 (0.228") - bigger number, smaller drill. Letter drills pick up where numbers leave off: A (0.234") through Z (0.413"), small to large. Both sets exist to fill the gaps between 1/64" fractional steps - and that's exactly why tap charts call out sizes like #7 or F: the fractional drills on either side would give too much or too little thread engagement. If your index only has fractions, pick the closest size and recompute the % with the formula up top before you commit.

How to read a thread callout

• 1/4-20 UNC-2B - quarter-inch nominal Ø, 20 threads per inch, Unified National Coarse, class 2B (internal, medium fit)
• M8 × 1.25 - 6H - 8 mm nominal Ø, 1.25 mm pitch, 6H tolerance class (internal, medium fit)
• 1/4-20 UNC-3B - same as 2B but tighter fit, used for safety-critical fasteners

2B is the default for most shop work. 3B is for aerospace or anything where backlash kills you. UNC is coarse (faster to assemble, better for soft material). UNF is fine (more threads per inch, holds tighter, better for vibration).

When to drop to 60% thread

• Stainless 304 / 316 - work hardens, taps break easy
• Titanium and Inconel - same story, plus heat
• Hardened tool steel - anything over Rc 30
• Blind holes deeper than 2× diameter - chip evacuation problems
• Hand-tapping in awkward fixtures - less torque to break the tap

At 60% thread engagement you've still got about ~95% of the holding strength of a 75% thread (yes, really - the curve flattens fast above 60%) but you've cut tap breakage way down. Production shops have known this for decades.

That's also why nobody drills for 100%: above ~75% the strength gains are nearly zero, but tapping torque - and tap breakage - climbs steeply. In stainless or titanium, drop to 60-65% and keep your taps. Full worked breakdown for one common size: 1/2-13 UNC tap drill at 75% engagement.

Worked example: 1/4-20 in 304 stainless

Material:    304 stainless (work-hardens, tough on taps)
Thread:      1/4-20 UNC
Strategy:    drop to 60% thread engagement

tap drill = 0.250 − 0.01299 × 60 / 20
          = 0.250 − 0.039
          = 0.211"

Closest standard drills: #4 (0.209" ≈ 63%) or #3 (0.213" ≈ 57%)
Pick #3 - err on the easy-tapping side in work-hardening material.
75% would have been #7 (0.201") - too tight for this material.

Common mistakes

• Using a 100% thread drill (the major diameter minus pitch) - the tap will fight you and probably snap.
• Forgetting peck depth on deep blind holes. Pull every 0.5–1× diameter to clear chips.
• Skipping the chamfer. A small countersink at the hole entrance keeps the tap straight.
• Tapping with no lubricant in stainless or aluminum. Tap Magic for steel, anhydrous IPA or kerosene for aluminum.

Run it on your phone

The ShopCalc app has a Tap Drill calculator that does this math for any thread (UNC/UNF/UNS/M-series) at any % engagement, plus the closest standard drill in either system. Plus speeds & feeds, drill chart, and metal weight. 100% offline, free on the App Store and Google Play.

Related

• How to calculate speeds and feeds for CNC machining
• 4140 steel milling — worked speeds/feeds for 1/4" carbide
• Trade calculator apps hub (ShopCalc + three other trades)
• ShopCalc: Machinist Calculator — free on iOS + Android
• Ace & Alan Tool — taps, end mills, drills

Note: Charts are starting points. Always verify against your tap manufacturer's recommended drill - a few makers (OSG, Emuge) publish their own charts that vary slightly for premium taps.