Tap drill chart and calculator.

01What a tap drill is and why percentage of thread matters

A tap cuts an internal thread into a hole that was drilled first. The drill sets the minor diameter of the thread, the size of the hole between the crests, and the tap cuts the flanks outward from there to the major diameter. Drill the hole at the major diameter and there is nothing left to cut; drill it at the theoretical root of a full sharp-V thread and the tap has to remove the whole thread form, which no one does because the tap would twist off. The tap drill sits between those two, and how far between is what the percentage of thread describes.

Percentage of thread is the share of the full thread height that is actually cut. The convention used for tap drill charts treats a 100% thread as one with a height of 0.6495 times the pitch on each side (three-quarters of the sharp-V height of 0.866P), so a 75% thread has a height of about 0.487P per side and a 50% thread about 0.325P. A smaller percentage means a larger hole, less metal for the tap to remove, lower torque, fewer broken taps and easier chip clearance. A larger percentage means a fuller thread with more flank contact.

The point that surprises people is how little strength the extra percentage buys. Machining references report that, with a normal length of engagement (about one diameter or more), the strength of the threaded joint rises only slightly between roughly 60% and 100% of thread, while the torque needed to drive the tap rises steeply. That is why the standard shop figure is 75% rather than something closer to full, and why the chart offers 50 and 60% as well: for tough materials you give up a little thread you did not need and keep the tap.

02The formula, inch and metric, with a worked example

Inch threads. Tap drill (in) = D − 0.01299 × % / TPI, where D is the basic major diameter in inches, % is the percentage of thread wanted (75, not 0.75) and TPI is threads per inch. The constant is 1.299 divided by 100: two thread heights of 0.6495P make 1.299P, and one per cent of that is 0.01299P, with P = 1/TPI.

Metric threads. Tap drill (mm) = D − (% / 76.98) × P, where D is the major diameter and P the pitch, both in millimetres. It is the same formula rearranged: 100 / 1.299 = 76.98, so at 75% it reduces to D − 0.974P.

Turned around, the same formula tells you what percentage a particular drill gives: % = (D − drill) × TPI / 0.01299 for inch, or % = (D − drill) / P × 76.98 for metric. That is the number in the chart's % thread column and in the calculator's tiles, and it is the form the arithmetic takes when the question is "what does this drill I have give me?"

Example 1: 1/2-13 UNC at 75% (the calculator's default)

D = 0.5000 in, TPI = 13. Tap drill = 0.5000 − 0.01299 × 75 / 13 = 0.5000 − 0.0749 = 0.4251 in (10.80 mm). The nearest standard drill is 27/64 at 0.4219 in, 0.0032 in under the calculated size, and it gives (0.5000 − 0.4219) × 13 / 0.01299 = 78.2%. The next size up, 7/16 (0.4375 in), gives 62.5%. Charts list 27/64 for 1/2-13 because it is the closest standard drill, and the thread it cuts is a few points fuller than 75%.

Example 2: M10 × 1.5 at 75%

D = 10 mm, P = 1.5 mm. Tap drill = 10 − (75 / 76.98) × 1.5 = 10 − 1.461 = 8.539 mm (0.3362 in). The nearest standard metric drill is 8.5 mm, which gives (10 − 8.5) / 1.5 × 76.98 = 77.0%. The D − P shop rule gives 8.5 mm for the same thread, which is the same drill.

Example 3: 3/8-16 UNC at 60% for a harder steel

D = 0.3750 in, TPI = 16, and the material calls for a lighter thread. Tap drill = 0.3750 − 0.01299 × 60 / 16 = 0.3750 − 0.0487 = 0.3263 in. Nearest standard drill: 21/64 at 0.3281 in, giving 57.7%. At 75% the same thread computes to 0.3141 in and the chart gives 5/16 at 77.0%, so dropping to 60% moves you up one fractional size, from 5/16 to 21/64.

03Why 75% is the default and when to use less

Seventy-five per cent is the figure most printed charts are built on and the one a tap maker assumes when it stamps a drill size on the tap's shank. It gives a full-looking thread that gauges properly, with a tapping torque that a hand tap or a machine tap in steel will tolerate. Unless a drawing, a specification or the material says otherwise, 75% is the answer.

Use less, 50 to 60%, when the tap is at risk or the material is hard to cut: alloy and tool steels, stainless steels, work-hardening nickel alloys, cast iron in small sizes, and deep or blind holes where chips pack. A 60% thread in a hard material is often stronger in practice than a 75% thread attempted with a tap that chatters, tears or breaks. Small taps (under about #10 or M5) break easily enough that many shops drop to 60 to 65% in steel as a matter of routine. The chart's 50 and 60% columns are computed with the same formula, so the drill they name is the nearest standard size to that lighter thread.

Use more than 75% only where the engagement is short and every thread counts: thin sheet, a tapped hole in a flange that is only half a diameter deep, or a soft material such as aluminium or brass, which taps easily and needs the extra flank contact because the thread itself is weak. Above about 80% the torque rises quickly; the calculator will take any percentage from 1 to 100, and prints the neighbouring drills so you can see what a size either way does.

Two cases the chart does not cover. Roll-form (fluteless) taps displace metal rather than cutting it and need a larger hole than a cutting tap for the same thread; use the tap maker's figure. And a threaded hole made to a drawing that calls up a thread class or a minor-diameter limit is inspected to that limit, not to a percentage, so the drill has to land inside the tolerance the drawing gives.

04Reading the chart: the nearest drill and the percentage it gives

The formula almost never lands on a drill you own. The chart shows the formula result, then the standard drill closest to it, above or below, and then the percentage of thread that drill actually cuts. Read the last column, not the heading: the heading says 75%, but the drill in the row gives whatever the arithmetic says, and it can be several points either side.

When the nearest drill is smaller than the calculated size, the thread comes out fuller. 1/2-13 UNC is the usual case: 27/64 gives 78.2% against the 75% asked for. When the nearest drill is larger, the thread comes out lighter. 3/4-10 UNC computes to 0.6526 in; the nearest standard drill is 21/32 at 0.6562 in, which gives 72.2%, and the next drill down, 41/64, would give 84.2%, which is more than most taps in steel want. The chart takes 21/32. 7/16-14 UNC is a near miss the other way: it computes to 0.3679 in and the letter U drill, 0.3680 in, sits less than a thousandth above it at 74.9%.

If the percentage in the row is further from your target than you like, the calculator shows the neighbouring drills. Enter the thread, and the tiles give the next drill down and the next drill up with the percentage each one produces, so you can choose the fuller or the lighter thread deliberately. "Snap to" lets you include metric drills for an inch thread or inch drills for a metric one; a 6.8 mm drill and a letter H drill are both real tools, and sometimes the other set has a closer size.

Number-size threads (#0 to #12) have their major diameter computed as 0.060 + 0.013 × the number, so #10 is 0.190 in and #6 is 0.138 in. Their tap drills are almost all number drills, which run the other way: a bigger number is a smaller drill (#80 is 0.0135 in, #1 is 0.228 in). Letter drills A to Z pick up from there (0.234 to 0.413 in) and fractional drills take over above that.

05Clearance drills

A clearance hole is not tapped. The bolt or screw passes through it and the thread is in the part behind, so the hole only has to be bigger than the major diameter of the fastener, by enough to allow for position error and the fastener's own tolerance. Drill a clearance hole at a tap drill size by mistake and the bolt will not go in; drill it at exactly the major diameter and it binds.

The chart's clearance column is a close fit, computed rather than copied. For inch sizes it is the smallest standard drill at or above the major diameter plus 2%: 1/2 in × 1.02 = 0.5100 in, and the next standard drill up is 33/64 (0.5156 in). For metric sizes it is the smallest standard metric drill at or above the major diameter plus 0.4 mm for M6 and larger, or plus 0.2 mm below M6, so M10 gets 10.4 mm and M12 gets 12.4 mm. The calculator prints the same figure for any thread you enter.

Treat it as a rule of thumb. The clearance-hole standards (ISO 273 for metric, ASME B18.2.8 for inch) list three series, usually called close, medium and coarse or normal and loose, and the medium and coarse figures are larger than this column, especially above M12 or 1/2 in. A drawing that specifies a clearance hole, or a hole that has to line up with others across a bolt pattern, uses the standard series or the drawing's own tolerance, not this column. Where nothing is specified and the parts are being fitted together on the bench, the close fit here is the usual starting point.

06Metric versus inch, and the D minus P rule

Metric threads are described by major diameter and pitch, the distance between threads, so the shop rule is simple: tap drill = D − P. M10 × 1.5 gives 8.5 mm, M8 × 1.25 gives 6.75 mm (use 6.8 mm), M12 × 1.75 gives 10.25 mm. Put D − P into the formula and it corresponds to a thread of 76.98%, call it 77%, so the rule and the 75% chart agree to within a tenth of a millimetre on nearly every size. Where they differ it is because of rounding to the 0.1 mm steps of the drill set: M12 × 1.75 computes to 10.295 mm at 75%, the nearest drill is 10.3 mm at 74.8%, and the 10.2 mm drill that D − P (10.25 mm) is usually rounded down to gives 79.2%. Either is a normal tap drill for M12; know which thread you are getting.

Inch threads are described by threads per inch, so there is no D − P to read off the designation, but the same rule holds if you convert: pitch = 1 / TPI. For 1/2-13, P = 0.0769 in and D − P = 0.4231 in, which again lands on 27/64. The 0.01299 formula is the general version of that rule with the percentage as a variable.

Drill sets differ. Metric drills step by 0.1 mm to 13 mm and by 0.5 mm above that, so a metric tap drill is usually within 0.05 mm of the formula. Inch sets are three overlapping series (numbers, letters, 64ths) that step unevenly, which is why some inch rows are several points off the target percentage and why letter and number drills exist at all: they fill the gaps between the fractions where the common taps fall. To convert between the two, 1 in = 25.4 mm exactly. The chart prints both units for every drill.

Do not mix the two systems on the same thread. An M10 × 1.5 tap in a 3/8 in hole (9.525 mm) gives about 24% of thread and the bolt will strip; a 3/8-16 tap in a 9 mm hole (0.3543 in) gives about 32%. Both look like a threaded hole until they are loaded.

07Common mistakes

• Drilling at the major diameter. A 1/2 in drill for a 1/2-13 tap leaves nothing to cut. The tap drill is always smaller than the nominal size of the thread; for 1/2-13 it is 27/64.
• Coarse drill for a fine thread, or the reverse. The same nominal diameter has a different tap drill for each pitch. 1/2-13 UNC takes 27/64; 1/2-20 UNF takes 29/64. M10 × 1.5 takes 8.5 mm; M10 × 1.25 takes 8.8 mm. Read the TPI or pitch off the tap or the drawing before you look up the drill.
• Too full a thread in hard material. Chasing 80 or 90% in alloy steel or stainless to make a "strong" thread mainly makes a broken tap. Drop to 60% and keep the engagement length.
• Confusing number and letter drills, or reading the number scale backwards. #7 is 0.201 in; letter F is 0.257 in; a #10 screw takes a #25 drill (0.1495 in) at 24 TPI, and the #10 drill itself (0.1935 in) is a different tool. Number drills get smaller as the number gets bigger.
• Tap drill in a clearance hole. A hole the bolt is meant to pass through needs the clearance drill, larger than the major diameter, not the tap drill.
• Using the wrong number size diameter. Number-size majors are 0.060 + 0.013 × n, so #8 is 0.164 in, not 0.180 in, and #12 is 0.216 in. Guessing the major from the nearest fraction puts the percentage off by ten points or more.
• Forgetting that the formula rounds to a real drill. The formula result is not a drill you can buy. Pick the nearest standard size, then work out what that size gives, and say that number if a question asks for the percentage.
• Per cent as a decimal. The 0.01299 form of the formula takes 75, not 0.75. Using 0.75 gives a drill within a thousandth of the major diameter.

08What the 433A exam expects

Threading and fastening sit in Block A of the Industrial Mechanic (Millwright) standard, common occupational skills, which our 433A exam guide sets out as 25 of the exam's 135 questions. Its largest task, routine trade tasks, lists fabricating a work piece, fastening and retaining devices and material identification among its sub-tasks; its tools and equipment task covers hand and portable power tools and shop machines; and measuring and layout covers laying out components and the precision measuring tools you would check a tapped hole with. Tap drills, drill sizes, thread designations and the difference between a tap drill and a clearance hole are the kind of fact a knowledge-and-recall question in that block is written to.

Block C, mechanical power transmission components and systems, is the largest at 32 questions, and its equipment tasks (shafts, bearings and seals; couplings, clutches and brakes; gear, chain and belt drives; prime movers) each have installs, diagnoses, maintains and repairs sub-tasks. Installing and repairing that equipment means drilling, tapping and bolting it down, and a repair question can turn on a damaged thread, a stripped hole, a helical insert (which needs its own, larger, tap drill) or a fastener that will not pass through a hole. The percentage-of-thread idea itself is a machining fact, and the same standard lists shop machines, including drill presses and lathes, under Block A.

Two things from the exam information page, as the guide reports them, are directly relevant. The acronym list provided with the exam includes tpi, and the formula sheet includes rpm from cutting speed and diameter, which is the calculation that follows tap-drill selection: once you have the drill size, the sheet's formula gives the spindle speed for it. The formula sheet does not include a tap drill formula, so if a question asks for one it is either a recall item (which drill for which tap) or gives you the numbers it wants you to use. Practise the 0.01299 form and the D − P rule until you can do either in a minute.

The guide also notes that the 433A question mix is 30 to 40% knowledge and recall and 40 to 50% procedural and application, which the Red Seal Exam Preparation Guide says can include calculations. Expect a tap drill question in either form: name the drill for a given thread, or compute a size from numbers in the stem. The free 433A questions include fastener and shop-practice items in the same format as the exam.

09Sources

• Red Seal Program: Industrial Mechanic (Millwright) trade page the trade the 433A exam certifies, the occupational standard editions, and links to the exam information page with the block breakdown, the formula sheet and the acronym list.
• ASME B1.1: Unified Inch Screw Threads (UN, UNR and UNJ thread forms) the standard that defines the UNC and UNF series, their basic major diameters and threads per inch. The metric series is ISO 261 (general-purpose metric screw threads, general plan). Both standards are copyrighted; this page reproduces no table from either. Every tap drill, percentage and clearance value here is computed from the percentage-of-thread formula and the standard number, letter, fractional and metric drill sizes.
• TicketPrep: 433A Industrial Mechanic (Millwright) Red Seal exam guide the block and task breakdown, the question-type mix, and the formula sheet and acronym list provided at the sitting.

10Questions people ask

What size drill do I use for a 1/2-13 tap?

A 27/64 drill (0.4219 in, 10.72 mm). The 75% formula gives 0.4251 in and 27/64 is the nearest standard drill; it cuts about 78% of thread. The next size up, 7/16, gives about 63%, which is a reasonable choice in hard steel. For 1/2-20 UNF the tap drill is 29/64.

What is the tap drill for M10 x 1.5?

8.5 mm (0.3346 in). The formula at 75% gives 8.539 mm, the nearest standard drill is 8.5 mm, and it cuts about 77% of thread. The shop rule D minus P gives the same answer: 10 minus 1.5 = 8.5 mm. For the M10 x 1.25 fine thread the tap drill is 8.8 mm.

What does 75% thread mean?

It means the tap cuts three-quarters of the full thread height, using the convention that a 100% thread has a height of 0.6495 times the pitch on each flank. The tap drill for 75% is D minus 0.01299 x 75 / TPI for inch threads or D minus 0.974 x pitch for metric threads. It is the standard shop figure because a fuller thread adds little strength with a normal engagement length but needs much more torque to tap. Harder materials are often tapped at 50 to 60%.

Can I just use major diameter minus pitch for a metric tap drill?

Yes for most work. D minus P corresponds to about 77% of thread, and after rounding to a standard 0.1 mm drill it gives the same drill as a 75% chart for nearly every size from M3 to M24. For an inch thread the equivalent is D minus 1/TPI. Where the two differ by one drill size, the chart's % thread column tells you what each one cuts.

Is a tap drill chart provided on the 433A Red Seal exam?

Not that the Red Seal Program lists. Its exam information page for Industrial Mechanic (Millwright) says a one-page formula sheet and an acronym list are provided with the exam; the formula sheet covers rigging, rpm from cutting speed and diameter, alignment shims, thermal expansion, areas and volumes, gear pass frequency and force from pressure and area, and the acronym list includes tpi. It does not include a tap drill formula or chart, so know the common sizes and the formula, and use the numbers a question gives you.

11Practice for this exam

Tap drills are one shop fact among hundreds on the 433A exam. TicketPrep 433A practice tests follow the Red Seal Program's block-by-block breakdown, and every answer is explained, including why each wrong option is wrong. You can try free sample questions with no account.

Ten free questions per trade, no account: free practice questions. How our questions are written and checked: how our questions are made.

Related guides