Free thread and drill reference

Tap drill size chart — at the engagement you choose

Every tap drill chart ever printed is one subtraction: the major diameter of the thread minus the engagement you want, times 1.29904, times the pitch. This page does the subtraction live for 65 UNC, UNF, metric coarse and metric fine threads, names the real bit that lands closest out of 305 fractional, number, letter and metric sizes, and tells you the percentage that bit truly gives rather than the one you asked for. Type a drill instead and it runs backwards: hand it a #7 and it lists every thread that bit can cut and how much of each.

100% free
No signup
65 threads
305 drill sizes
75% and 50% columns

Thread

Thread engagement

Charts print 75%. Between 60% and 75% you are mostly buying tapping torque rather than joint strength; under about 50% the thread does start giving up load it cannot spare.

Tap drill for 1/4-20 at 75%

#70.201 in

Exact diameter: 0.2013 in / 5.11 mm
That bit really gives: 75.4%
Closest metric bit: 5.1 mm at 75.8%
Clearance, close fit: 0.257 in
Clearance, normal fit: 0.266 in

0.25 in major, minus 75% of 0.065 in of full-thread depth, is 0.2013 in. The depth term is 1.29904 × pitch — twice 0.64952 P — the full-thread depth a 60° Unified or ISO profile is measured against in the standard tap drill formula.

Filter the chart

Units

65 of 65 threads shown. Printing takes exactly these rows, so filter to the series you actually cut before you hit print.

Tap drill and clearance drill sizes for Unified and metric threads
		Pitch		Tap drill, 50%	Clearance, close	Clearance, normal
#0-80UNF	0.06 in	80 TPI	3/64 (0.0469 in)	#55 (0.052 in)	0.067 in	0.073 in
#1-64UNC	0.073 in	64 TPI	#53 (0.0595 in)	1/16 (0.0625 in)	0.0785 in	0.081 in
#1-72UNF	0.073 in	72 TPI	#53 (0.0595 in)	#52 (0.0635 in)	0.0785 in	0.081 in
#2-56UNC	0.086 in	56 TPI	#50 (0.07 in)	#49 (0.073 in)	0.089 in	0.096 in
#2-64UNF	0.086 in	64 TPI	#50 (0.07 in)	#48 (0.076 in)	0.089 in	0.096 in
#3-48UNC	0.099 in	48 TPI	#47 (0.0785 in)	#44 (0.086 in)	0.1015 in	0.1065 in
#3-56UNF	0.099 in	56 TPI	#45 (0.082 in)	#44 (0.086 in)	0.1015 in	0.1065 in
#4-40UNC	0.112 in	40 TPI	#43 (0.089 in)	#41 (0.096 in)	0.116 in	0.1285 in
#4-48UNF	0.112 in	48 TPI	#42 (0.0935 in)	#40 (0.098 in)	0.116 in	0.1285 in
#5-40UNC	0.125 in	40 TPI	#38 (0.1015 in)	7/64 (0.1094 in)	0.1285 in	0.136 in
#5-44UNF	0.125 in	44 TPI	#37 (0.104 in)	#35 (0.11 in)	0.1285 in	0.136 in
#6-32UNC	0.138 in	32 TPI	#36 (0.1065 in)	#32 (0.116 in)	0.144 in	0.1495 in
#6-40UNF	0.138 in	40 TPI	#33 (0.113 in)	#31 (0.12 in)	0.144 in	0.1495 in
#8-32UNC	0.164 in	32 TPI	#29 (0.136 in)	#27 (0.144 in)	0.1695 in	0.177 in
#8-36UNF	0.164 in	36 TPI	#29 (0.136 in)	#26 (0.147 in)	0.1695 in	0.177 in
#10-24UNC	0.19 in	24 TPI	#25 (0.1495 in)	#20 (0.161 in)	0.196 in	0.201 in
#10-32UNF	0.19 in	32 TPI	#21 (0.159 in)	#18 (0.1695 in)	0.196 in	0.201 in
#12-24UNC	0.216 in	24 TPI	#16 (0.177 in)	#12 (0.189 in)	0.221 in	0.228 in
#12-28UNF	0.216 in	28 TPI	#14 (0.182 in)	#10 (0.1935 in)	0.221 in	0.228 in
1/4-20UNC	0.25 in	20 TPI	#7 (0.201 in)	7/32 (0.2188 in)	0.257 in	0.266 in
1/4-28UNF	0.25 in	28 TPI	#3 (0.213 in)	#1 (0.228 in)	0.257 in	0.266 in
5/16-18UNC	0.3125 in	18 TPI	F (0.257 in)	J (0.277 in)	0.323 in	0.332 in
5/16-24UNF	0.3125 in	24 TPI	I (0.272 in)	9/32 (0.2813 in)	0.323 in	0.332 in
3/8-16UNC	0.375 in	16 TPI	5/16 (0.3125 in)	Q (0.332 in)	0.386 in	0.397 in
3/8-24UNF	0.375 in	24 TPI	Q (0.332 in)	S (0.348 in)	0.386 in	0.397 in
7/16-14UNC	0.4375 in	14 TPI	U (0.368 in)	25/64 (0.3906 in)	0.4531 in	0.4687 in
7/16-20UNF	0.4375 in	20 TPI	25/64 (0.3906 in)	Y (0.404 in)	0.4531 in	0.4687 in
1/2-13UNC	0.5 in	13 TPI	27/64 (0.4219 in)	29/64 (0.4531 in)	0.5156 in	0.5312 in
1/2-20UNF	0.5 in	20 TPI	29/64 (0.4531 in)	15/32 (0.4688 in)	0.5156 in	0.5312 in
9/16-12UNC	0.5625 in	12 TPI	31/64 (0.4844 in)	33/64 (0.5156 in)	0.5781 in	0.5937 in
9/16-18UNF	0.5625 in	18 TPI	33/64 (0.5156 in)	17/32 (0.5313 in)	0.5781 in	0.5937 in
5/8-11UNC	0.625 in	11 TPI	17/32 (0.5313 in)	9/16 (0.5625 in)	0.6406 in	0.6562 in
5/8-18UNF	0.625 in	18 TPI	37/64 (0.5781 in)	19/32 (0.5938 in)	0.6406 in	0.6562 in
3/4-10UNC	0.75 in	10 TPI	21/32 (0.6563 in)	11/16 (0.6875 in)	0.7656 in	0.7812 in
3/4-16UNF	0.75 in	16 TPI	11/16 (0.6875 in)	45/64 (0.7031 in)	0.7656 in	0.7812 in
7/8-9UNC	0.875 in	9 TPI	49/64 (0.7656 in)	51/64 (0.7969 in)	0.8906 in	0.9062 in
7/8-14UNF	0.875 in	14 TPI	13/16 (0.8125 in)	53/64 (0.8281 in)	0.8906 in	0.9062 in
1-8UNC	1 in	8 TPI	7/8 (0.875 in)	59/64 (0.9219 in)	1.0156 in	1.0312 in
1-12UNF	1 in	12 TPI	59/64 (0.9219 in)	61/64 (0.9531 in)	1.0156 in	1.0312 in
M2 × 0.4coarse	0.0787 in	0.4 mm	1.6 mm	1.7 mm	0.0866 in	0.0945 in
M2 × 0.25fine	0.0787 in	0.25 mm	1.8 mm	1.8 mm	0.0866 in	0.0945 in
M2.5 × 0.45coarse	0.0984 in	0.45 mm	2.1 mm	2.2 mm	0.1063 in	0.1142 in
M2.5 × 0.35fine	0.0984 in	0.35 mm	2.2 mm	2.3 mm	0.1063 in	0.1142 in
M3 × 0.5coarse	0.1181 in	0.5 mm	2.5 mm	2.7 mm	0.126 in	0.1339 in
M3 × 0.35fine	0.1181 in	0.35 mm	2.7 mm	2.8 mm	0.126 in	0.1339 in
M4 × 0.7coarse	0.1575 in	0.7 mm	3.3 mm	3.5 mm	0.1693 in	0.1772 in
M4 × 0.5fine	0.1575 in	0.5 mm	3.5 mm	3.7 mm	0.1693 in	0.1772 in
M5 × 0.8coarse	0.1969 in	0.8 mm	4.2 mm	4.5 mm	0.2087 in	0.2165 in
M5 × 0.5fine	0.1969 in	0.5 mm	4.5 mm	4.7 mm	0.2087 in	0.2165 in
M6 × 1coarse	0.2362 in	1 mm	5.0 mm	5.4 mm	0.252 in	0.2598 in
M6 × 0.75fine	0.2362 in	0.75 mm	5.3 mm	5.5 mm	0.252 in	0.2598 in
M8 × 1.25coarse	0.315 in	1.25 mm	6.8 mm	7.2 mm	0.3307 in	0.3543 in
M8 × 1fine	0.315 in	1 mm	7.0 mm	7.4 mm	0.3307 in	0.3543 in
M10 × 1.5coarse	0.3937 in	1.5 mm	8.5 mm	9.0 mm	0.4134 in	0.4331 in
M10 × 1.25fine	0.3937 in	1.25 mm	8.8 mm	9.2 mm	0.4134 in	0.4331 in
M12 × 1.75coarse	0.4724 in	1.75 mm	10.3 mm	10.9 mm	0.5118 in	0.5315 in
M12 × 1.25fine	0.4724 in	1.25 mm	10.8 mm	11.2 mm	0.5118 in	0.5315 in
M14 × 2coarse	0.5512 in	2 mm	12.1 mm	12.7 mm	0.5906 in	0.6102 in
M14 × 1.5fine	0.5512 in	1.5 mm	12.5 mm	13.0 mm	0.5906 in	0.6102 in
M16 × 2coarse	0.6299 in	2 mm	14.0 mm	14.5 mm	0.6693 in	0.689 in
M16 × 1.5fine	0.6299 in	1.5 mm	14.5 mm	15.0 mm	0.6693 in	0.689 in
M20 × 2.5coarse	0.7874 in	2.5 mm	17.5 mm	18.5 mm	0.8268 in	0.8661 in
M20 × 1.5fine	0.7874 in	1.5 mm	18.5 mm	19.0 mm	0.8268 in	0.8661 in
M24 × 3coarse	0.9449 in	3 mm	21.0 mm	22.0 mm	0.9843 in	1.0236 in
M24 × 2fine	0.9449 in	2 mm	22.0 mm	22.5 mm	0.9843 in	1.0236 in

Tap drills are computed, not transcribed: major diameter minus engagement × 1.29904 × pitch, then rounded to the nearest bit in a fractional, number, letter or tenth-millimeter set. Clearance holes are the close and normal columns of ASME B18.2.8 for Unified sizes and ISO 273 for metric. The one figure here that is a judgment rather than a standard is the tapping-torque penalty: tap makers' published torque comparisons between a 60% and a 75% thread in the same hole, roughly 2× going from 60% to 75%, and it moves with material, tap geometry and coating, hole depth, and whether the hole is blind.

How to pick a tap drill

The chart is the easy part. Choosing what percentage of thread to cut is the decision.

Pick the thread, not the drill
Choose the thread you are cutting from the list — #10-24 and #10-32 share a major diameter and want holes 0.010 in apart, so the series matters as much as the size. Metric rows carry their pitch in the name, because M8 on its own is ambiguous: coarse is 1.25 mm and fine is 1.0 mm, and the tap drills differ by two tenths.
Set how much thread you actually want
Seventy-five percent is what every printed chart assumes, and it is a poor default in tough material or a blind hole. Drop it to 65% or 60% and the recommended bit changes; the panel then tells you what percentage that bit really delivers, which is never exactly the number you asked for because drills come in fixed steps.
Read the bit, the clearance hole and the shortfall
The result names a bit you can pull out of an index — #7, letter F, 27/64, 6.8 mm — with the exact computed diameter beside it and the engagement it lands on. It also gives the closest bit from the other measurement system for the common case of an inch tap and a metric index, plus the close and normal clearance holes for the piece the fastener passes through.

Technical specifications

Threads listed	65 — 19 UNC and 20 UNF from #0 to 1 in, plus 13 metric coarse and 13 metric fine from M2 to M24
Engagement range	30% to 100%, with 50, 60, 65, 70, 75 and 85 as one-tap presets
Drill index	305 sizes: fractional in 64ths, number drills #1–#60, letter drills A–Z, and metric 1.0–14.0 mm in tenths plus 14.5–26.0 mm in half steps
Formula	drill = major diameter − (engagement ÷ 100) × 1.29904 × pitch, where 1.29904 is twice the 0.64952 P full-thread depth
Clearance holes	ASME B18.2.8 close and normal for Unified sizes; ISO 273 close and medium for metric
Reverse lookup	Accepts #7, F, 13/64, 0.201 and 5.2 mm; returns every thread that bit lands between 45% and 100% on
Print output	Nav, ads and prose drop out; the printed sheet carries only the rows left by your filter
Data kept	None — the table is generated in the tab and nothing you type is transmitted

Frequently asked questions

What is the tap drill for 1/4-20?

A #7 bit, 0.201 in. The arithmetic is 0.250 major diameter minus 75% of 1.29904 × 0.05 pitch, which is 0.2013, and #7 is the nearest bit in a standard index at 0.201. In fractional sizes only, 13/64 (0.2031) is the next best thing and lands you at about 72% thread — a difference no bolt in a 1/4-20 hole will ever notice.

Why do two tap drill charts disagree about the same thread?

Because they assume different thread engagement and usually do not print which. A chart aimed at production shops quotes 60% to 65% to keep taps alive; a chart aimed at general repair quotes 75%; some hand-tool charts quote a bit as large as 85% for aluminum. All three are correct for the assumption behind them, which is exactly why the engagement is a control on this page rather than a hidden constant.

Is a 75% thread meaningfully stronger than a 60% one?

Barely, and not in the way that decides a joint. Thread shear area scales roughly with engagement, so 60% carries about four fifths of what 75% carries — but a tapped hole one and a half diameters deep is already stronger than the bolt going into it, so the bolt snaps first in both cases. What does change dramatically is the torque the tap has to survive: tap makers put the increase from 60% to 75% at around double, and a snapped tap in a finished part is a much more expensive problem than a thread at 60%.

Can I drill an inch thread with a metric bit, or the other way round?

Yes, and the panel gives you the closest bit from the other system with the engagement it produces. A 3.8 mm drill in a #10-24 hole lands at 74.6% against the 74.8% of the #25 the chart names, and no thread will ever know the difference. The case to be careful about is a fine pitch on a small size, where a tenth of a millimeter moves the engagement a long way: on #4-48 the step from a 2.4 mm bit to a 2.5 mm bit drops it from 65% to 50%, so check the exact diameter rather than trusting the nearest bit.

What size hole does the bolt itself pass through?

The clearance columns, and they are not the same as the tap drill. Close fit is a hole barely larger than the major diameter — 0.257 in for a 1/4 in bolt, 6.4 mm for an M6 — for joints that have to stay located. Normal fit adds another few thousandths so parts can be assembled without a reamer. Using the tap drill as a clearance hole is the classic way to end up cutting a thread in the piece that was supposed to slide.

Does this chart cover NPT pipe threads?

No, and no percentage-of-engagement chart can. NPT is a tapered thread cut into a tapered reamed hole, so the drill size comes from the tap manufacturer's own table rather than from a formula on major diameter and pitch — 1/8 NPT wants 11/32 or letter R depending on how deep the fitting is meant to run in. Treat pipe taps as a separate lookup.

Do thread-forming taps use these numbers?

No — a form tap needs a distinctly larger hole, because it displaces metal rather than cutting it away and the displaced material has to go somewhere. An M6 × 1 rolled to about 65% starts from 5.6 mm, where the cutting tap on this chart asks for 5.0 mm at 75%; the difference is six tenths of a millimeter, not a rounding step, and every tap maker publishes the exact figure for its own geometry. The trade-off is worth taking in ductile material: no chips, a thread with the grain flow bent round it rather than cut through, and no broken tap to fish out of a blind hole.

About thread engagement and where 75% came from

A tapped hole is not a thread with a percentage attached — it is a hole of a particular diameter, and the percentage is just a way of describing how far short of the theoretical root that hole falls. Drill exactly to the minor diameter of a 60° thread and you get 100%: full crests, no clearance, and a tap that has to remove every scrap of metal between the two. Drill larger and the crests get flattened off; at 75% a quarter of the theoretical thread height is simply not there. The published constant behind the whole business is 0.64952 × pitch, the depth of the fundamental triangle per side, which doubles to 1.29904 across the diameter. Every chart on the internet is that number with a percentage in front of it.

Seventy-five percent became the default for a reason that no longer applies to most people using it: it is a comfortable compromise for a production tap in free-machining steel, cutting dry, where the tap is a consumable and the part is not. In a one-off aluminum bracket held in a drill press, it is the wrong end of the trade. Shear area grows roughly in step with engagement, so dropping to 60% gives up about a fifth of the thread strength — except that a hole tapped a diameter and a half deep already fails by snapping the bolt rather than stripping, which means the fifth you gave up was strength the joint could never use. Meanwhile the metal the tap has to shift, and with it the torque, climbs steeply. That is the actual choice this page is built to expose, and it is why the engagement here is a control rather than a hidden assumption.

The other half of the job is the hole the fastener passes through, which is why the clearance columns sit next to the tap drills. Confusing the two is the most common way a two-plate joint goes wrong: thread both plates and they jack apart instead of clamping. For wood the equivalent pair is the pilot and the shank hole, worked out by gauge and species on the screw size chart, and for anything driven rather than turned there is no hole at all — the nail size chart covers the penny system that sizes those instead. If the threads in question are holding a structure together rather than a machine, the fastening schedule matters more than the drill: start from the rafter calculator for the cut list and take the connection detail from your local code.

Where this chart is generated

Every number on this page is worked out by JavaScript running in the tab you are reading it in. Nothing you type — measurements, quantities, the prices your supplier quoted you — is uploaded, logged or kept, which is also why the calculators carry on working on a site with no signal.

There is no lookup table on a server here to be queried — the 65 threads and 305 drill sizes are a few kilobytes of JavaScript, and every diameter you see was multiplied out on your own device the moment the page loaded.