Drill Size Chart: Metric, Number and Letter Drills

Why there are four drill designations

Every drill chart exists because of a gap. Four systems are in use at the same time, and none of them was designed to be converted into the others.

The metric series steps in 0.1 mm. Below 13 mm that is the whole system: a standard metric drill set is 1.0 mm to 13.0 mm in 0.1 mm increments.

The fractional inch series steps in 64ths, from 1/64 in upward. It is the oldest of the four and the coarsest.

The number series, #1 to #80, and the letter series, A to Z, were created by the American machine tool industry to fill the gaps the fractional series left. A 64th of an inch is 0.397 mm, which is far too wide a step when the part has to work. So the trade produced a set of drills at sizes in between and named them by number and letter rather than by dimension.

The result is that four designations can land on nearly the same hole, and the chart is the only way to see how nearly. The important consequence is that a number or a letter is a name, not a measurement. A #7 drill is not seven of anything; it is 0.2010 in. A letter drill is not coarse or fine as a class; it is one of twenty-six sizes that happen to fall between the number series and the larger fractional sizes.

Metric drill sizes

This is the table for metric work, and it is the one that matters if the drawing is dimensioned in millimetres. The list is the standard metric drill set from 1.0 mm to 13.0 mm in 0.1 mm steps, continued above 13 mm in 0.5 mm steps.

The inch column is a conversion, not a commercial size. The inch is defined as exactly 25.4 mm, so a 5.0 mm drill is 0.1969 in by definition and there is nothing approximate about it. What is approximate is the fit: no inch drill is made to 5.0 mm except a 5.0 mm drill.

Metric drill (mm)	Inch decimal
1.0	0.0394
1.1	0.0433
1.2	0.0472
1.3	0.0512
1.4	0.0551
1.5	0.0591
1.6	0.0630
1.7	0.0669
1.8	0.0709
1.9	0.0748
2.0	0.0787
2.1	0.0827
2.2	0.0866
2.3	0.0906
2.4	0.0945
2.5	0.0984
2.6	0.1024
2.7	0.1063
2.8	0.1102
2.9	0.1142
3.0	0.1181
3.1	0.1220
3.2	0.1260
3.3	0.1299
3.4	0.1339
3.5	0.1378
3.6	0.1417
3.7	0.1457
3.8	0.1496
3.9	0.1535
4.0	0.1575
4.1	0.1614
4.2	0.1654
4.3	0.1693
4.4	0.1732
4.5	0.1772
4.6	0.1811
4.7	0.1850
4.8	0.1890
4.9	0.1929
5.0	0.1969
5.1	0.2008
5.2	0.2047
5.3	0.2087
5.4	0.2126
5.5	0.2165
5.6	0.2205
5.7	0.2244
5.8	0.2283
5.9	0.2323
6.0	0.2362
6.1	0.2402
6.2	0.2441
6.3	0.2480
6.4	0.2520
6.5	0.2559
6.6	0.2598
6.7	0.2638
6.8	0.2677
6.9	0.2717
7.0	0.2756
7.1	0.2795
7.2	0.2835
7.3	0.2874
7.4	0.2913
7.5	0.2953
7.6	0.2992
7.7	0.3031
7.8	0.3071
7.9	0.3110
8.0	0.3150
8.1	0.3189
8.2	0.3228
8.3	0.3268
8.4	0.3307
8.5	0.3346
8.6	0.3386
8.7	0.3425
8.8	0.3465
8.9	0.3504
9.0	0.3543
9.1	0.3583
9.2	0.3622
9.3	0.3661
9.4	0.3701
9.5	0.3740
9.6	0.3780
9.7	0.3819
9.8	0.3858
9.9	0.3898
10.0	0.3937
10.1	0.3976
10.2	0.4016
10.3	0.4055
10.4	0.4094
10.5	0.4134
10.6	0.4173
10.7	0.4213
10.8	0.4252
10.9	0.4291
11.0	0.4331
11.1	0.4370
11.2	0.4409
11.3	0.4449
11.4	0.4488
11.5	0.4528
11.6	0.4567
11.7	0.4606
11.8	0.4646
11.9	0.4685
12.0	0.4724
12.1	0.4764
12.2	0.4803
12.3	0.4843
12.4	0.4882
12.5	0.4921
12.6	0.4961
12.7	0.5000
12.8	0.5039
12.9	0.5079
13.0	0.5118
13.5	0.5315
14.0	0.5512
14.5	0.5709
15.0	0.5906
15.5	0.6102
16.0	0.6299
16.5	0.6496
17.0	0.6693
17.5	0.6890
18.0	0.7087
18.5	0.7283
19.0	0.7480
19.5	0.7677
20.0	0.7874

Above about 13 mm the table thins out, and that is not an omission. Large holes are rarely drilled. A 20 mm twist drill needs a spindle with the torque to turn it and the rigidity to keep it straight, and the hole it leaves still needs finishing if it has to be accurate. Most shops interpolate a large hole with an end mill on a CNC milling machine instead, which gives a rounder, better-controlled hole from tooling that is already in the machine.

Number drill sizes, #1 to #80

The number series is the workhorse of inch-based small-hole work. The numbering runs backwards, which catches people out: #80 is the smallest at 0.0135 in, and #1 is the largest at 0.2280 in. A bigger number is a smaller drill.

Number drill	Decimal (in)	Metric (mm)
1	0.2280	5.791
2	0.2210	5.613
3	0.2130	5.410
4	0.2090	5.309
5	0.2055	5.220
6	0.2040	5.182
7	0.2010	5.105
8	0.1990	5.055
9	0.1960	4.978
10	0.1935	4.915
11	0.1910	4.851
12	0.1890	4.801
13	0.1850	4.699
14	0.1820	4.623
15	0.1800	4.572
16	0.1770	4.496
17	0.1730	4.394
18	0.1695	4.305
19	0.1660	4.216
20	0.1610	4.089
21	0.1590	4.039
22	0.1570	3.988
23	0.1540	3.912
24	0.1520	3.861
25	0.1495	3.797
26	0.1470	3.734
27	0.1440	3.658
28	0.1405	3.569
29	0.1360	3.454
30	0.1285	3.264
31	0.1200	3.048
32	0.1160	2.946
33	0.1130	2.870
34	0.1110	2.819
35	0.1100	2.794
36	0.1065	2.705
37	0.1040	2.642
38	0.1015	2.578
39	0.0995	2.527
40	0.0980	2.489
41	0.0960	2.438
42	0.0935	2.375
43	0.0890	2.261
44	0.0860	2.184
45	0.0820	2.083
46	0.0810	2.057
47	0.0785	1.994
48	0.0760	1.930
49	0.0730	1.854
50	0.0700	1.778
51	0.0670	1.702
52	0.0635	1.613
53	0.0595	1.511
54	0.0550	1.397
55	0.0520	1.321
56	0.0465	1.181
57	0.0430	1.092
58	0.0420	1.067
59	0.0410	1.041
60	0.0400	1.016
61	0.0390	0.991
62	0.0380	0.965
63	0.0370	0.940
64	0.0360	0.914
65	0.0350	0.889
66	0.0330	0.838
67	0.0320	0.813
68	0.0310	0.787
69	0.0292	0.742
70	0.0280	0.711
71	0.0260	0.660
72	0.0250	0.635
73	0.0240	0.610
74	0.0225	0.571
75	0.0210	0.533
76	0.0200	0.508
77	0.0180	0.457
78	0.0160	0.406
79	0.0145	0.368
80	0.0135	0.343

Two things are worth noticing in that table. The spacing is not even: the series is denser at the small end, where a small absolute difference in diameter is a large relative one, and it opens out as the sizes grow. And the whole series sits below 6 mm, which is why it is mostly encountered on small parts — instrument fittings, small fasteners, injector and manifold work, and the fine end of precision machining.

Letter drill sizes, A to Z

The letter series picks up where the number series runs out. It starts at A, 0.2340 in, and ends at Z, 0.4130 in, with the fractional sizes interleaved among them. Several letters are standard tap drills for inch threads — F is the tap drill for a 5/16-18 thread, for example.

Letter drill	Decimal (in)	Metric (mm)
A	0.2340	5.944
B	0.2380	6.045
C	0.2420	6.147
D	0.2460	6.248
E	0.2500	6.350
F	0.2570	6.528
G	0.2610	6.629
H	0.2660	6.756
I	0.2720	6.909
J	0.2770	7.036
K	0.2811	7.140
L	0.2900	7.366
M	0.2950	7.493
N	0.3020	7.671
O	0.3160	8.026
P	0.3230	8.204
Q	0.3320	8.433
R	0.3390	8.611
S	0.3480	8.839
T	0.3580	9.093
U	0.3680	9.347
V	0.3770	9.576
W	0.3860	9.804
X	0.3970	10.084
Y	0.4040	10.262
Z	0.4130	10.490

A letter drill is often the nearest thing to a metric size that an inch toolroom will have on the shelf. That is useful, and it is also the trap covered further down: the nearest equivalent is not the same size.

Fractional drill sizes

The fractional series is the one most people meet first, and it is the coarsest. Sixty-fourths run from 1/64 in to 1 in, and above about 1/2 in most shops stop stocking every 64th and interpolate instead.

Fractional drill	Decimal (in)	Metric (mm)
1/64 in	0.0156	0.397
1/32 in	0.0313	0.794
3/64 in	0.0469	1.191
1/16 in	0.0625	1.587
5/64 in	0.0781	1.984
3/32 in	0.0938	2.381
7/64 in	0.1094	2.778
1/8 in	0.1250	3.175
9/64 in	0.1406	3.572
5/32 in	0.1563	3.969
11/64 in	0.1719	4.366
3/16 in	0.1875	4.762
13/64 in	0.2031	5.159
7/32 in	0.2188	5.556
15/64 in	0.2344	5.953
1/4 in	0.2500	6.350
17/64 in	0.2656	6.747
9/32 in	0.2813	7.144
19/64 in	0.2969	7.541
5/16 in	0.3125	7.938
21/64 in	0.3281	8.334
11/32 in	0.3438	8.731
23/64 in	0.3594	9.128
3/8 in	0.3750	9.525
25/64 in	0.3906	9.922
13/32 in	0.4063	10.319
27/64 in	0.4219	10.716
7/16 in	0.4375	11.112
29/64 in	0.4531	11.509
15/32 in	0.4688	11.906
31/64 in	0.4844	12.303
1/2 in	0.5000	12.700
33/64 in	0.5156	13.097
17/32 in	0.5313	13.494
35/64 in	0.5469	13.891
9/16 in	0.5625	14.287
37/64 in	0.5781	14.684
19/32 in	0.5938	15.081
39/64 in	0.6094	15.478
5/8 in	0.6250	15.875
41/64 in	0.6406	16.272
21/32 in	0.6563	16.669
43/64 in	0.6719	17.066
11/16 in	0.6875	17.462
45/64 in	0.7031	17.859
23/32 in	0.7188	18.256
47/64 in	0.7344	18.653
3/4 in	0.7500	19.050
49/64 in	0.7656	19.447
25/32 in	0.7813	19.844
51/64 in	0.7969	20.241
13/16 in	0.8125	20.637
53/64 in	0.8281	21.034
27/32 in	0.8438	21.431
55/64 in	0.8594	21.828
7/8 in	0.8750	22.225
57/64 in	0.8906	22.622
29/32 in	0.9063	23.019
59/64 in	0.9219	23.416
15/16 in	0.9375	23.813
61/64 in	0.9531	24.209
31/32 in	0.9688	24.606
63/64 in	0.9844	25.003
1 in	1.0000	25.400

The trap in most drill charts

Most drill charts published online have a column called something like nearest equivalent, sitting next to a column called decimal size, with the two behaving differently from row to row. In the same table, one row’s decimal column can hold the true size of the fractional drill named in that row, while the next row’s decimal column holds the inch conversion of a metric size rather than the size of the number drill named beside it.

Read the second kind of row literally and you conclude that a #60 drill is 0.0394 in and therefore exactly 1.0 mm. It is not. A #60 drill is 0.0400 in, or 1.016 mm, and 1.0 mm is 0.0394 in. The two are close, and they are not the same size — the difference is 0.016 mm, which is more than the general tolerance band on a small dimension under ISO 2768-m.

The rule that avoids the whole problem is to read a drill chart for one thing only: the actual size of the designation. If a chart also wants to tell you the nearest equivalent, that belongs in a column that says so, and it should never be the column a machinist reads a dimension from.

The same discipline applies to the metric to inch conversion of a drawing dimension. Converting a number is arithmetic; substituting a drill is a decision about the hole.

The hole is not the drill size

This is the part a drill chart cannot tell you, and it is the part that causes the most scrapped parts.

A twist drill is a cutting tool. It removes material by pushing a wedge through it, and the hole it leaves is the result of that process rather than a copy of the tool. Four things push the hole off nominal, and they all push it the same way — a drilled hole comes out oversize.

• Point geometry and web thickness. The chisel edge at the centre of the drill does not cut; it extrudes. That alone disturbs the hole at the point of entry.
• Lip height mismatch. The two cutting edges are never perfectly equal, so one does more work than the other and the drill is pushed sideways as it cuts.
• Runout. Chuck, collet or holder runout is multiplied down the length of the drill, and a long drill amplifies it.
• Deflection and material behaviour. The drill bends under load, and materials spring back differently. Soft aluminium and plastics move more than steel; work-hardening stainless moves in its own way.

The practical figures are worth carrying in your head. In steel, a drilled hole typically finishes 0.02 to 0.1 mm oversize, and the spread widens with depth and with the length-to-diameter ratio of the drill. In soft aluminium and in plastics it is larger. In cast iron it can be smaller, because the material breaks rather than deforms.

What follows from that is a rule about drawing: a hole that has to fit something is not a drilled hole. It is drilled undersize and then reamed, bored or interpolated by an end mill, which puts the final size under the control of a tool guided by the existing hole rather than one that makes it. The diameters, fits and callouts for that are set out on the tolerances page.

Choosing a size for the job the hole has to do

A drill size is chosen from what the hole is for, and there are only four answers.

A clearance hole. The fastener passes through and nothing else depends on the size. This is where the nearest equivalent is fine and where being 0.05 mm off costs nothing. Clearance holes are the case that makes the whole approximate-equivalents idea survivable.

A tap drill. The hole has to leave the right amount of material for the thread to cut into. The size comes from the thread standard, not from the drill chart: nominal diameter minus pitch for a metric thread, and the equivalent tables for unified threads. The drill chart’s job is only to confirm what that size is. The full set is on threaded holes: depth and drill size, and the designations themselves are on thread standards.

A reamed or bored hole. The drill is a roughing tool and the size that matters is the finished one. The rule of thumb is to leave 0.1 to 0.3 mm of material for a reamer, which means drilling a size that does not appear in the chart at all as a finished dimension — it is an intermediate, not the hole.

A press fit or interference fit. Such a hole is not drilled to size at all. It is produced by reaming or boring to a tolerance band that is a fraction of the interference, and the drill size only decides how much material is left to remove.

Getting the left-hand column right on the drawing — see drawing and file requirements — is what makes the drill size a shop decision rather than a specification.

What changes on the shop floor

The chart gives a size. What a shop does with it depends on four things, and none of them changes the number.

The material. A 304 stainless part and a 6061 aluminium part at the same hole size are not the same job. Stainless work-hardens, so a drill that rubs instead of cutting hardens the surface it has to cut through and dulls twice as fast; free-machining grades such as 303 and 416 exist for exactly that reason. Aluminium galls and builds up on the cutting edge, so it wants more clearance and a sharper edge. Plastics melt, so they want a drill ground for the material and enough feed to get through before the heat builds.

The depth. A hole deeper than about three times its diameter needs peck drilling to clear chips, and past about five times the diameter the drill starts to wander even with care. That is when a shop interpolates a pilot and then finishes the hole by another route.

The point angle. A 118 degree point is the general-purpose geometry, 135 degrees is used for harder materials and for thinner sections, and a 90 degree point is for sheet and for the seat of a countersunk fastener. The point angle changes how the drill enters, which changes how far the hole is off at entry.

The number of holes. One hole is a setup. A thousand holes is a tool life exercise, and the last hundred will not be the same size as the first fifty unless the drill is changed on a count. Any part that runs in volume — the sort of work that fills a large CNC machining envelope or a secondary operations bench — is planned around that.

What to put on the drawing

The cleanest way to make all of this somebody else’s problem is to specify holes rather than drills.

Instead of	Write
A drill size	The hole diameter, with its tolerance and its depth
A callout for a tap drill	The thread designation, and let the shop pick the tap drill
Twelve undimensioned holes marked M6	The tap drill, the thread and the depth, or the thread and a depth that implies them
A drilled hole called out as a fit	Drill undersize and ream or bore, stated as such
Depth left off	Depth, or through — with the material thickness the through hole has to clear
A nearest equivalent	The size you actually want, in the system the drawing is dimensioned in

The reason to reverse the instinct is simple. If the drawing names a drill, the drawing has fixed the process and the shop has to either follow it or come back with a question. If the drawing names the hole, the shop can choose whichever route gets there most cheaply — and the hole is what the part needed all along.

Where the drill chart stops

A drill chart answers one question: how big is this drill. It does not answer how big the hole will be, whether the hole will be round, whether it will be straight, or how deep it can go before the drill wanders. Those are process questions, and they are settled by the material, the depth, the tool and the setup.

The useful habit is to read the chart for sizes, the thread standard for tap drills, and the tolerance page for everything that has to fit. Keep the three separate and the numbers stay honest.

Send the drawing with the holes dimensioned, and it comes back within 24 hours with a quote and DFM feedback — including a note where a hole carries a tolerance its function does not need, which is the least expensive change a design can make. We hold plus or minus 0.01 mm where it is required, with ISO 2768-m as the general tolerance block, and mill envelopes up to 800 by 500 mm. Orders start at 50 pieces per style and material, samples from a single piece in 5 to 10 days, production in 25 to 35 days, and every batch ships with a material certificate (MTR) tracing the grade to its mill heat plus pre-shipment photographs. Start from the request a quote page, or see what else we machine on the materials index.