Reference

Tap Drill Size Chart

The drill to use before tapping every common inch, metric, and pipe thread, with decimal and millimeter sizes, the percent thread each drill gives, and clearance holes for the mating screw.

A tap drill is the hole you drill before cutting an internal thread with a tap. It is sized slightly larger than the thread's minor diameter so the tap cuts roughly 75% of a full thread, which keeps nearly all of the thread's strength while taking far less tapping torque than a full-depth thread.

Quick answers: 1/4-20 uses a #7 drill (0.201 in). 10-32 uses a #21 (0.159 in). 8-32 uses a #29 (0.136 in). 3/8-16 uses a 5/16" drill. M6 x 1 uses a 5.0 mm drill. For metric coarse threads, the tap drill is the nominal diameter minus the pitch.

The tables below cover the full UNC, UNF, metric coarse, metric fine, and NPT pipe thread ranges. Every inch row lists the percent thread that drill produces, so you can see how close it lands to the 75% target. To size a hole for a drill number or letter on its own, see the drill size chart.

Most common tap drill sizes

The threads that show up on most drawings, in one place. Full tables for each thread series follow.

Thread	Tap drill	Decimal (in)	Decimal (mm)
#4-40 UNC	#43	0.0890	2.26
#6-32 UNC	#36	0.1065	2.71
#8-32 UNC	#29	0.1360	3.45
#10-24 UNC	#25	0.1495	3.80
#10-32 UNF	#21	0.1590	4.04
1/4-20 UNC	#7	0.2010	5.11
1/4-28 UNF	#3	0.2130	5.41
5/16-18 UNC	F	0.2570	6.53
3/8-16 UNC	5/16"	0.3125	7.94
1/2-13 UNC	27/64"	0.4219	10.72
M3 x 0.5	2.5 mm	0.0984	2.50
M4 x 0.7	3.3 mm	0.1299	3.30
M5 x 0.8	4.2 mm	0.1654	4.20
M6 x 1.0	5.0 mm	0.1969	5.00
M8 x 1.25	6.8 mm	0.2677	6.80
M10 x 1.5	8.5 mm	0.3346	8.50
M12 x 1.75	10.2 mm	0.4016	10.20
1/8 NPT	R	0.3390	8.61
1/4 NPT	7/16"	0.4375	11.11

Cutting-tap drills at about 75% thread. NPT sizes are for tapping without a taper pipe reamer.

UNC tap drill chart (Unified coarse)

Coarse threads are the default for most screws and bolts. They tap faster, tolerate burrs and plating better, and strip less easily in soft materials like aluminum.

Thread	Tap drill	Decimal (in)	Decimal (mm)	Thread %
#1-64 UNC	#53	0.0595	1.51	67%
#2-56 UNC	#50	0.0700	1.78	69%
#3-48 UNC	#47	0.0785	1.99	76%
#4-40 UNC	#43	0.0890	2.26	71%
#5-40 UNC	#38	0.1015	2.58	72%
#6-32 UNC	#36	0.1065	2.71	78%
#8-32 UNC	#29	0.1360	3.45	69%
#10-24 UNC	#25	0.1495	3.80	75%
#12-24 UNC	#16	0.1770	4.50	72%
1/4-20 UNC	#7	0.2010	5.11	75%
5/16-18 UNC	F	0.2570	6.53	77%
3/8-16 UNC	5/16"	0.3125	7.94	77%
7/16-14 UNC	U	0.3680	9.35	75%
1/2-13 UNC	27/64"	0.4219	10.72	78%
9/16-12 UNC	31/64"	0.4844	12.30	72%
5/8-11 UNC	17/32"	0.5313	13.49	79%
3/4-10 UNC	21/32"	0.6563	16.67	72%
7/8-9 UNC	49/64"	0.7656	19.45	76%
1-8 UNC	7/8"	0.8750	22.23	77%

Thread % is calculated as (major diameter - drill) x TPI / 0.01299 and shows how close the nearest standard drill lands to the 75% target.

UNF tap drill chart (Unified fine)

Fine threads have more threads per inch, which gives finer adjustment, better resistance to loosening under vibration, and more thread engagement in thin walls.

Thread	Tap drill	Decimal (in)	Decimal (mm)	Thread %
#0-80 UNF	3/64"	0.0469	1.19	81%
#1-72 UNF	#53	0.0595	1.51	75%
#2-64 UNF	#50	0.0700	1.78	79%
#3-56 UNF	#45	0.0820	2.08	73%
#4-48 UNF	#42	0.0935	2.37	68%
#5-44 UNF	#37	0.1040	2.64	71%
#6-40 UNF	#33	0.1130	2.87	77%
#8-36 UNF	#29	0.1360	3.45	78%
#10-32 UNF	#21	0.1590	4.04	76%
#12-28 UNF	#14	0.1820	4.62	73%
1/4-28 UNF	#3	0.2130	5.41	80%
5/16-24 UNF	I	0.2720	6.91	75%
3/8-24 UNF	Q	0.3320	8.43	79%
7/16-20 UNF	25/64"	0.3906	9.92	72%
1/2-20 UNF	29/64"	0.4531	11.51	72%
9/16-18 UNF	33/64"	0.5156	13.10	65%
5/8-18 UNF	37/64"	0.5781	14.68	65%
3/4-16 UNF	11/16"	0.6875	17.46	77%
7/8-14 UNF	13/16"	0.8125	20.64	67%
1-12 UNF	59/64"	0.9219	23.42	72%

For 9/16-18 and 5/8-18, no standard drill lands near 75%: the listed drill gives about 65% thread, and the next size down (1/2" and 9/16") gives about 87%. Some charts, including Machinery's Handbook, list the smaller drill. 1"-14 (a common UNS fine thread) taps with a 15/16" drill at about 67%.

Metric coarse tap drill chart (ISO)

For metric coarse threads, tap drill (mm) = nominal diameter - pitch. M8 x 1.25 works out to 6.75 mm, so shops use the standard 6.8 mm drill. The closest inch drill is listed for shops that stock number, letter, and fractional drills.

Thread	Pitch (mm)	Tap drill (mm)	Decimal (in)	Closest inch drill
M1.6 x 0.35	0.35	1.25	0.0492	No close match
M2 x 0.4	0.4	1.6	0.0630	1/16" (0.0625)
M2.5 x 0.45	0.45	2.05	0.0807	#46 (0.0810)
M3 x 0.5	0.5	2.5	0.0984	#40 (0.0980)
M3.5 x 0.6	0.6	2.9	0.1142	#33 (0.1130)
M4 x 0.7	0.7	3.3	0.1299	#30 (0.1285)
M5 x 0.8	0.8	4.2	0.1654	#19 (0.1660)
M6 x 1.0	1.0	5.0	0.1969	#9 (0.1960)
M8 x 1.25	1.25	6.8	0.2677	H (0.2660)
M10 x 1.5	1.5	8.5	0.3346	Q (0.3320)
M12 x 1.75	1.75	10.2	0.4016	Y (0.4040)
M14 x 2.0	2.0	12.0	0.4724	15/32" (0.4688)
M16 x 2.0	2.0	14.0	0.5512	35/64" (0.5469)
M18 x 2.5	2.5	15.5	0.6102	39/64" (0.6094)
M20 x 2.5	2.5	17.5	0.6890	11/16" (0.6875)
M22 x 2.5	2.5	19.5	0.7677	49/64" (0.7656)
M24 x 3.0	3.0	21.0	0.8268	53/64" (0.8281)
M27 x 3.0	3.0	24.0	0.9449	15/16" (0.9375)
M30 x 3.5	3.5	26.5	1.0433	1-3/64" (1.0469)

Metric sizes follow ISO 261 coarse pitches. An inch substitute is listed only when it lands between about 65% and 85% thread.

Metric fine tap drill chart (ISO)

Fine-pitch metric threads use the same rule, nominal minus pitch, so a smaller pitch means a larger tap drill. M10 x 1.0 uses a 9.0 mm drill, while M10 x 1.5 coarse uses 8.5 mm.

Thread	Pitch (mm)	Tap drill (mm)	Decimal (in)	Closest inch drill
M8 x 1.0	1.0	7.0	0.2756	J (0.2770)
M10 x 1.25	1.25	8.8	0.3465	S (0.3480)
M10 x 1.0	1.0	9.0	0.3543	T (0.3580)
M12 x 1.5	1.5	10.5	0.4134	Z (0.4130)
M12 x 1.25	1.25	10.8	0.4252	27/64" (0.4219)
M14 x 1.5	1.5	12.5	0.4921	No close match
M16 x 1.5	1.5	14.5	0.5709	37/64" (0.5781)
M18 x 1.5	1.5	16.5	0.6496	21/32" (0.6563)
M20 x 1.5	1.5	18.5	0.7283	47/64" (0.7344)
M22 x 1.5	1.5	20.5	0.8071	13/16" (0.8125)
M24 x 2.0	2.0	22.0	0.8661	55/64" (0.8594)

NPT pipe thread tap drill chart

NPT threads are tapered (1 in 16 on diameter) and seal on the thread flanks with sealant or tape. Pipe sizes are nominal: a 1/8 NPT thread is about 0.405 in across, not 1/8 in.

Pipe size	Threads per inch	Tap drill	Decimal (in)	Decimal (mm)
1/8 NPT	27	R	0.3390	8.61
1/4 NPT	18	7/16"	0.4375	11.11
3/8 NPT	18	37/64"	0.5781	14.68
1/2 NPT	14	23/32"	0.7188	18.26
3/4 NPT	14	59/64"	0.9219	23.42
1 NPT	11.5	1-5/32"	1.1563	29.37

Sizes for tapping without a taper pipe reamer, per Machinery's Handbook. Reaming the hole to the taper first lets you start with a slightly smaller drill and reduces tapping torque.

Tap drill formula

To size a tap drill for any thread or percent thread:

Inch threads: tap drill = major diameter - (0.01299 x percent thread / TPI). For 1/4-20 at 75%: 0.250 - (0.01299 x 75 / 20) = 0.201 in, a #7 drill.
Metric threads: tap drill = nominal diameter - (percent thread x pitch / 76.98). At about 77% thread this reduces to nominal minus pitch, which is why M6 x 1 uses a 5.0 mm drill.

Choosing a percent thread: 75% is the standard target. Going above it adds little strength but raises tapping torque sharply, which breaks taps in tough materials. Many shops drop to about 60-65% in stainless, titanium, and hardened steel, and when the thread engagement length is at least 1.5 times the diameter.

Forming (roll) taps displace material instead of cutting it, so they need a larger drill than the sizes on this page. Use the tap maker's forming-tap chart.

Inch clearance holes (close and free fit)

A clearance hole lets a screw pass through a part without threading into it. Close fit locates the part more accurately; free fit leaves room for hole-position error between mating parts.

Screw size	Close fit drill	Close (in)	Free fit drill	Free (in)
#0	#52	0.0635	#50	0.0700
#2	#43	0.0890	#41	0.0960
#4	#32	0.1160	#30	0.1285
#6	#27	0.1440	#25	0.1495
#8	#18	0.1695	#16	0.1770
#10	#9	0.1960	#7	0.2010
#12	#2	0.2210	#1	0.2280
1/4	F	0.2570	H	0.2660
5/16	P	0.3230	Q	0.3320
3/8	W	0.3860	X	0.3970
7/16	29/64"	0.4531	15/32"	0.4688
1/2	33/64"	0.5156	17/32"	0.5313
5/8	41/64"	0.6406	21/32"	0.6563
3/4	49/64"	0.7656	25/32"	0.7813
1	1-1/64"	1.0156	1-1/32"	1.0313

Common shop values. For critical fits, check hole sizes against ASME B18.2.8.

Metric clearance holes (ISO 273)

ISO 273 defines three clearance hole series for metric fasteners. Medium (normal) is the usual default.

Screw size	Fine (mm)	Medium (mm)	Coarse (mm)
M1.6	1.7	1.8	2.0
M2	2.2	2.4	2.6
M2.5	2.7	2.9	3.1
M3	3.2	3.4	3.6
M4	4.3	4.5	4.8
M5	5.3	5.5	5.8
M6	6.4	6.6	7.0
M8	8.4	9.0	10.0
M10	10.5	11.0	12.0
M12	13.0	13.5	14.5
M14	15.0	15.5	16.5
M16	17.0	17.5	18.5
M20	21.0	22.0	24.0
M24	25.0	26.0	28.0

Inch tap drills follow the standard 75%-thread chart, metric tap drills follow nominal minus pitch, NPT sizes follow Machinery's Handbook, and metric clearance holes follow ISO 273. Confirm thread class, material, and depth for your part before cutting.

On OpenSpindle

Frequently Asked Questions

What size drill do I use for a 1/4-20 tap?

Use a #7 drill (0.201 in, 5.11 mm) for a 1/4-20 UNC thread. It gives about 75% thread. A 13/64 in drill (0.203 in) is a close substitute if you do not have a #7.

What is the tap drill size for 10-32?

Use a #21 drill (0.159 in, 4.04 mm) for a 10-32 UNF thread, which gives about 76% thread. For 10-24 UNC, use a #25 drill (0.1495 in).

What is the tap drill size for 8-32?

Use a #29 drill (0.136 in, 3.45 mm) for 8-32 UNC. The same #29 drill is used for 8-36 UNF.

What size drill for a 3/8-16 tap?

Use a 5/16 in drill (0.3125 in, 7.94 mm) for 3/8-16 UNC. For 3/8-24 UNF, use a letter Q drill (0.332 in).

What is the tap drill size for 5/16-18?

Use a letter F drill (0.257 in, 6.53 mm) for 5/16-18 UNC. For 5/16-24 UNF, use a letter I drill (0.272 in).

What size drill for a 6-32 tap?

Use a #36 drill (0.1065 in, 2.71 mm) for 6-32 UNC. For 6-40 UNF, use a #33 drill (0.113 in).

What is the tap drill size for 1/2-13?

Use a 27/64 in drill (0.4219 in, 10.72 mm) for 1/2-13 UNC. For 1/2-20 UNF, use a 29/64 in drill (0.4531 in).

What is the tap drill size for M6, M8, and M10?

M6 x 1.0 uses a 5.0 mm drill, M8 x 1.25 uses a 6.8 mm drill, and M10 x 1.5 uses an 8.5 mm drill. For any metric coarse thread, tap drill = nominal diameter minus pitch.

What size drill for a 1/8 NPT tap?

Use a letter R drill (0.339 in, 8.61 mm) for 1/8-27 NPT when tapping without a reamer. A 1/4 NPT thread uses a 7/16 in drill.

How do I calculate tap drill size?

For inch threads, tap drill = major diameter - (0.01299 x percent thread / threads per inch). For metric threads, tap drill = nominal diameter - (percent thread x pitch / 76.98), which simplifies to nominal minus pitch at about 77% thread.

What is 75% thread engagement?

It is the depth of thread the tap cuts compared with a theoretical full (100%) thread. A 75% thread keeps nearly all the strength of a full thread while cutting much less material, so it is the standard target on tap drill charts. Deeper threads add little strength and raise the risk of breaking the tap.

What is the difference between a tap drill and a clearance hole?

A tap drill is slightly larger than the thread's minor diameter so the hole can be tapped. A clearance hole is larger than the screw's major diameter so the screw passes through freely. For example, a 1/4-20 screw uses a #7 tap drill in the threaded part and an F (close) or H (free) clearance drill in the part it passes through.

Send your drawing with the threads and holes called out, and set a budget. We source machine shops and bring back a best-match quote.

Get quotes for machined parts