Find the drill size before tapping a metric or UNC/UNF inch thread, for cutting and forming taps, or the thread percentage a given drill gives.

The forming tap drill comes from D − 0.0068 × % × P (percentage on the 0.6495P basis), the formula tap makers commonly use. Each maker's figure differs a little; use the catalogue of the tap you actually use.

How it is calculated

What thread percentage means

A cutting tap does not enlarge the hole: it cuts the thread groove into the wall of the drilled hole, so the crests of the internal thread are exactly at the drilled wall. The smaller the hole, the further the crests reach toward the axis and the deeper they engage the bolt's thread. Thread percentage (percentage of thread, thread engagement) gives the height of this internal thread against a reference height. This page follows the Japanese standard JIS B 1004, which takes the basic engagement height $H_1 = 0.5413\,P$ per side as 100%.

One side of an internal thread in axial section (the hole's axis is below). With a

D - P

tap drill, the crests of the internal thread are cut flat at the drilled wall. The dashed lines are the part of the basic profile that is not formed, and the fundamental triangle is

H = 0.866\,P

high.

H_1 = \tfrac{5}{8}H = 0.5413\,P

is the basic engagement height from D to D1, the 100% of JIS B 1004. The root of the internal thread is a flat

P/8

wide at D; the crest of the basic profile is a flat

P/4

wide at D1. With the

D - P

drill the real crest is a little wider, about

0.3\,P

The thread is on both sides of the hole, so the drilled diameter is smaller than $D$ by twice the thread height, and the formula is

d_{\text{drill}} = D - \frac{\%}{100} \times 1.0825\,P \qquad \% = \frac{D - d_{\text{drill}}}{1.0825\,P} \times 100

where

$d_{\text{drill}}$ is the tap drill size (mm)
$D$ is the nominal diameter of the thread (mm), such as 8 mm for M8
$P$ is the pitch (mm)
$\%$ is the thread percentage
$1.0825\,P$ is twice the basic engagement height $H_1 = 0.5413\,P = \tfrac{5}{8}H$ , where $H = 0.866\,P$ is the height of the metric thread's fundamental triangle

Every percentage on this page is on this JIS B 1004 basis unless it is marked 0.6495P. Tap drill charts and machinists' handbooks from the United States, used alongside the ASME inch thread standards, mostly take a taller reference height of $0.6495\,P$ , which gives a number 1.2 times smaller for the same hole; see two kinds of thread percentage below.

Where the reference height comes from

Every thread starts from the fundamental triangle: an equilateral 60° triangle as wide as the pitch, so $H = \tfrac{\sqrt{3}}{2}P = 0.866\,P$ high. A real thread has no sharp tips: the triangle's crest and root are cut off flat, so the thread height depends on how much the standard takes off at each.

The ISO basic profile, which JIS and the ASME Unified thread share, has a flat $P/8$ wide at the root of the internal thread (at D), taking $H/8$ off the height, and a flat $P/4$ wide at its crest (at D1), taking $H/4$ off. What is left is the height over which the external and internal threads overlap, the basic engagement height

H_1 = H - \tfrac{H}{8} - \tfrac{H}{4} = \tfrac{5}{8}H = 0.5413\,P

JIS B 1004 calls the percentage the engagement rate (ひっかかり率) and takes this height as 100%, so a hole of exactly $D_1 = D - 1.0825\,P$ is 100% thread. The other heights compare with it as follows.

Height per side	Value	JIS B 1004	0.6495P basis
Fundamental triangle (sharp) $H$	$0.866\,P$	160%	133%
American National thread $\tfrac{3}{4}H$ (the 0.6495P basis)	$0.6495\,P$	120%	100%
ISO external thread, to the rounded root $\tfrac{17}{24}H$	$0.6134\,P$	113%	94%
ISO internal thread, basic profile $\tfrac{5}{8}H$ (drill = D1, reference height)	$0.5413\,P$	100%	83%
Drill $D - P$	$0.5\,P$	92%	77%

So 100% is the full profile of the internal thread. Going past 100% does not make the thread any taller: the tap has to cut metal off the crests as well, which adds torque without adding strength. The calculator warns when the drill is smaller than D1.

On the other side, the standard lets the internal thread's minor diameter be larger than D1 within its tolerance. M8 class 6H, for example, allows a minor diameter from 6.647 to 6.912 mm, about 80% to 100% thread (see the tolerance tables below). The 6.8 mm drill (89%) sits right in the middle; a hole larger than the upper limit gives a thread out of tolerance.

Thread percentage allowed by the tolerance class

Thread standards do not give a thread percentage. They set limits on the minor diameter of the internal thread, and those limits are a percentage range. The smallest minor diameter allowed is D1 itself, always 100% (83% on the 0.6495P basis): a smaller hole is out of tolerance, and the tap has to cut the crests. The largest is D1 + TD1, where TD1 is the minor diameter tolerance. It gives the lowest percentage allowed, which depends on the pitch and the tolerance class. The table gives the minor diameter limits and the percentage range for ISO metric internal threads of class 6H (ISO 965-1). The minor diameter column is for the example thread in each row, from D1 to D1 + TD1.

Pitch P (mm)	e.g.	Minor diameter, 6H (mm)	JIS B 1004	0.6495P basis
0.35	M1.6	1.221 – 1.321	74% – 100%	61% – 83%
0.4	M2	1.567 – 1.679	74% – 100%	62% – 83%
0.45	M2.5	2.013 – 2.138	74% – 100%	62% – 83%
0.5	M3	2.459 – 2.599	74% – 100%	62% – 83%
0.7	M4	3.242 – 3.422	76% – 100%	64% – 83%
0.8	M5	4.134 – 4.334	77% – 100%	64% – 83%
1	M6	4.917 – 5.153	78% – 100%	65% – 83%
1.25	M8	6.647 – 6.912	80% – 100%	67% – 83%
1.5	M10	8.376 – 8.676	82% – 100%	68% – 83%
1.75	M12	10.106 – 10.441	82% – 100%	69% – 83%
2	M14	11.835 – 12.210	83% – 100%	69% – 83%
2.5	M18	15.294 – 15.744	83% – 100%	69% – 83%
3	M24	20.752 – 21.252	85% – 100%	71% – 83%
3.5	M30	26.211 – 26.771	85% – 100%	71% – 83%
4	M36	31.670 – 32.270	86% – 100%	72% – 83%
4.5	M42	37.129 – 37.799	86% – 100%	72% – 83%
5	M48	42.587 – 43.297	87% – 100%	72% – 83%
5.5	M56	50.046 – 50.796	87% – 100%	73% – 83%
6	M64	57.505 – 58.305	88% – 100%	73% – 83%

6H is the usual class for nuts and tapped holes; 5H has a narrower range and 7H a wider one, and the calculator above checks any of them. The percentage range depends only on the pitch, not the diameter, so M8 and M10×1.25 share it. The common D − P drill (92%) is inside this range at every pitch. The 60% to 78% often suggested for hard materials is below the 6H limit at most pitches: the thread may well be strong enough, but its minor diameter is over the 6H limit, which a plain plug gauge finds and a thread plug gauge does not.

Unified internal threads of classes 1B and 2B (ASME B1.1), 1/4 in and larger, have a minor diameter tolerance of 0.25P − 0.4P² (P = 1/TPI in), which gives these ranges:

Thread	Minor diameter (in)	JIS B 1004	0.6495P basis
1/4-20 UNC	0.1959 – 0.2074	79% – 100%	66% – 83%
5/16-18 UNC	0.2524 – 0.2650	79% – 100%	66% – 83%
3/8-16 UNC	0.3073 – 0.3214	79% – 100%	66% – 83%
7/16-14 UNC	0.3602 – 0.3760	80% – 100%	66% – 83%
1/2-13 UNC	0.4167 – 0.4336	80% – 100%	66% – 83%
9/16-12 UNC	0.4723 – 0.4903	80% – 100%	67% – 83%
5/8-11 UNC	0.5266 – 0.5460	80% – 100%	67% – 83%
3/4-10 UNC	0.6417 – 0.6627	81% – 100%	67% – 83%
7/8-9 UNC	0.7547 – 0.7776	81% – 100%	68% – 83%
1-8 UNC	0.8647 – 0.8897	82% – 100%	68% – 83%
1-1/8-7 UNC	0.9704 – 0.9979	82% – 100%	68% – 83%
1-1/4-7 UNC	1.0954 – 1.1229	82% – 100%	68% – 83%
1-3/8-6 UNC	1.1946 – 1.2251	83% – 100%	69% – 83%
1-1/2-6 UNC	1.3196 – 1.3501	83% – 100%	69% – 83%
1/4-28 UNF	0.2113 – 0.2198	78% – 100%	65% – 83%
5/16-24 UNF	0.2674 – 0.2771	78% – 100%	65% – 83%
3/8-24 UNF	0.3299 – 0.3396	78% – 100%	65% – 83%
7/16-20 UNF	0.3834 – 0.3949	79% – 100%	66% – 83%
1/2-20 UNF	0.4459 – 0.4574	79% – 100%	66% – 83%
9/16-18 UNF	0.5024 – 0.5150	79% – 100%	66% – 83%
5/8-18 UNF	0.5649 – 0.5775	79% – 100%	66% – 83%
3/4-16 UNF	0.6823 – 0.6964	79% – 100%	66% – 83%
7/8-14 UNF	0.7977 – 0.8135	80% – 100%	66% – 83%
1-12 UNF	0.9098 – 0.9278	80% – 100%	67% – 83%
1-1/8-12 UNF	1.0348 – 1.0528	80% – 100%	67% – 83%
1-1/4-12 UNF	1.1598 – 1.1778	80% – 100%	67% – 83%
1-3/8-12 UNF	1.2848 – 1.3028	80% – 100%	67% – 83%
1-1/2-12 UNF	1.4098 – 1.4278	80% – 100%	67% – 83%

Class 3B has a tighter tolerance, and sizes below 1/4 in follow other rules, so the calculator does not check them. Note also that the drilled hole is not exactly the minor diameter of the thread: a drill usually cuts a little oversize, and in soft materials the tap pushes some metal back into the hole. Check a critical thread both ways: a Go/No-go thread plug gauge checks the pitch diameter and functional size (the Go plug also confirms the major diameter is not too small), and a Go/No-go plain plug gauge checks the minor diameter.

Which percentage to choose

92% thread gives a drill of about $D - P$ , the rule every machinist knows: M8 takes a 6.8 mm drill. Figures widely quoted from American handbooks say that 75% thread on the 0.6495P basis (90% here) carries some 95% of the load of a full thread but needs only about a third of the tapping torque of 100% on that basis (120% here). A higher percentage adds very little strength and much more risk of breaking the tap, since a thread long enough (about 1 to 1.5 × D in steel) is usually stronger than the bolt already.

60% to 78% (0.6495P basis 50% to 65%): hard or tough materials that are difficult to cut, such as stainless steel and titanium, or threads deeper than 1.5 × D
78% to 92% (0.6495P basis 65% to 77%): general work in steel and aluminium
92% to 100% (0.6495P basis 77% to 83%): soft materials such as cast aluminium or plastics, or short threads in thin sheet, where as much thread as possible is wanted

Two kinds of thread percentage: JIS B 1004 and 0.6495P

Not every table means the same thing by thread percentage. This calculator takes 100% as the basic engagement height $H_1 = 0.5413\,P$ per side, as in JIS B 1004 (hole sizes before threading) and as above. Tap drill charts and machinists' handbooks from the United States mostly take 100% as $0.6495\,P = \tfrac{3}{4}H$ per side instead. That is the height of the American National thread, the forerunner of the Unified thread, which had flats $P/8$ wide at both crest and root. The charts kept this height as 100% after the thread standard changed: the Unified thread of ASME B1.1 has the same basic profile as the ISO metric thread, with an internal thread only $\tfrac{5}{8}H$ high, so on the 0.6495P basis a full-profile thread is 83% and a 100% thread cannot be made.

\%_{0.6495P} = \frac{D - d_{\text{drill}}}{1.299\,P} \times 100 = \frac{\%}{1.2}

Both formulas describe the same hole; only the number differs, by a factor of exactly 1.2. M8 with a 6.8 mm drill is 89% by JIS and 74% on the 0.6495P basis. The danger is mixing the two: a chart from an American source that asks for 65% to 75% thread means 78% to 90% on this page. Putting 75% into the JIS formula gives a hole that is too large: for M8 it is a 6.99 mm hole, above the 6.912 mm limit of class 6H. The forming tap makers' formula below is written for the 0.6495P basis too. Choose the basis in the calculator to match the table you are comparing with; the other figure is always shown alongside. The drawing below compares the two profiles.

Both profiles are to the same scale (the hole's axis is below), and each panel gives the percentages on its own basis. Top: the American National thread has flats

P/8

wide at both crest and root, so its internal thread is

\tfrac{3}{4}H = 0.6495\,P

high, and American charts call that 100%. Bottom: the ISO profile used by JIS and by ASME B1.1 keeps the root but cuts the crest back to a flat

P/4

wide at D1, leaving

\tfrac{5}{8}H = 0.5413\,P

, which JIS B 1004 calls 100%. The dashed tip is the

H/8

of the American National crest that no longer exists, the difference between 100% and 120%.

Forming taps

A forming tap does not cut: it presses the hole wall so the metal flows up into the crests. The metal pressed down into the groove becomes the crest reaching toward the axis, so the tap drill is much larger than for a cutting tap. Tap makers use

d_{\text{drill}} = D - 0.0068 \times \%_{0.6495P} \times P = D - 0.00567 \times \% \times P

The makers write the formula for the 0.6495P percentage; the second form is the same formula for the JIS percentage used on this page. The thread percentage here means the same as for a cutting tap: the height of the finished thread, measured to the tips of the crests, against $H_1$ . Put another way, it gives the minor diameter of the formed thread, $\approx D - \tfrac{\%}{100} \times 1.0825\,P$ . M8 at 78%, for example, has a minor diameter of about 6.94 mm, the same as a cutting tap at 78%. What differs is the drill: a cutting tap is drilled to the minor diameter wanted, while a forming tap is drilled larger and pushes the metal in to that level. The drawing below compares 78% thread from both taps.

Both drawings are to the same scale (the hole's axis is below). Top: the cutting tap cuts the groove into the drilled wall, so the crest is exactly at the wall. Bottom: the forming tap starts from a larger hole; metal pushed out of the groove flows up the flanks into a crest with two tips that reach the same 78% level, but there is not enough metal to fill the crest, so a split is left in the middle (split crest). The split is drawn with the area of the metal that is missing against a full crest; its real shape depends on the material and the tap.

The split crest is normal for a formed thread; the lower the percentage, the deeper the split. At about 120% (100% on the 0.6495P basis) the formula gives a drill of $D - 0.68\,P$ , close to the pitch diameter $D_2 = D - 0.6495\,P$ , where there is enough metal to fill the crest and the split closes. A formed thread carries the load on its flanks like a cut thread, so the split at the crest costs little strength. The 0.0068 is an experimental figure from the tap makers, and differs a little between them.

Most makers recommend 55% to 75% on the 0.6495P basis for formed threads, which is 66% to 90% here; this calculator starts at 78% (65% on the 0.6495P basis), which for M8 gives a 7.45 mm hole and a 7.4 mm drill. Since the percentage means the same thing, the minor diameter tolerance applies to formed threads too: M8 class 6H needs at least about 80% thread (the exact figure depends on the pitch). The default 78% gives a minor diameter slightly over the limit, but rounded to a 7.4 mm drill it gives about 85%, which is within it. If the work must meet 6H, check the minor diameter against this range with a plain plug gauge; a thread plug gauge checks the pitch diameter, not the minor diameter. Forming too high a thread leaves the metal nowhere to go, and the torque rises until the tap may break; drilling only slightly undersize matters much more than with a cutting tap. Use the values from the catalogue of the tap you actually use. Forming taps suit ductile materials that can stretch, such as low-carbon steel, stainless steel, aluminium and copper, not cast iron or brittle materials.

Inch threads (UNC and UNF)

Unified inch threads (ASME B1.1) have the same 60° basic profile as ISO metric threads, so the same formulas apply with the pitch $P = 25.4 / \text{TPI}$ mm. Worked in inches, the formula is

d_{\text{drill}} = D - \frac{0.010825 \times \%}{\text{TPI}} \qquad \% = \frac{\text{TPI} \times (D - d_{\text{drill}})}{0.010825}

and for forming taps $d_{\text{drill}} = D - 0.00567 \times \% / \text{TPI}$ . American tap drill charts usually print percentages on the 0.6495P basis instead, with 0.01299 in place of 0.010825 and 0.0068 in place of 0.00567: the roughly 75% such a chart gives for 1/4-20 UNC with a #7 drill is about 90% here. Choose the 0.6495P basis in the calculator to compare with those charts. At 92% the calculator shows the drill from the usual tap drill table, such as #7 for 1/4-20 UNC. At other percentages it picks the nearest number, letter or fractional drill, and also the nearest metric drill for shops that only have metric drills. In the drill to percentage mode, an inch drill can be typed as a decimal in inches or by its name, such as #7, F or 27/64. Unified internal threads use classes 1B, 2B and 3B instead of 6H, so the minor diameter limits differ from the metric figures above; see UNC and UNF inch threads.

Tap drill size