What percentage of thread actually means
Percentage of thread is the fraction of the theoretical full thread depth that the tap forms in your hole. It is a linear measure on diameter, not an area or a volume. Drill the hole exactly to the thread's minor diameter and the tap cuts a full-form thread, 100%. Drill it larger and the crests of the internal thread are simply missing — there is no material there for the tap to reach.
Everything about tap drill selection follows from one asymmetry. Tapping torque rises rapidly as engagement increases, because the tap has to remove more material per flute and the friction between the tap flanks and the hole grows. Thread strength rises far more slowly, because in a properly proportioned joint the thread is not what fails — a steel bolt in a steel nut of standard height breaks in tension long before the threads strip. The result is that pushing engagement from 75% toward 100% buys very little strength and costs a great deal of torque, which is why 75% became the general-purpose standard and why nobody drills to the minor diameter.
The engagement you can afford also depends on how much thread length you have. A blind hole in aluminium two diameters deep has plenty of thread to share the load and can run at 60% quite happily. A 0.060 in thick sheet has room for one or two threads, and there the extra engagement genuinely matters.
Where the constants 1.29904 and 1.0825 come from
Both unified and ISO metric threads use a 60° symmetrical form derived from a sharp V triangle of height H = 0.866025 × pitch. The standards then truncate that triangle at the crest and root, and for the internal thread the material removed on each side of the axis is 0.625 H = 0.541266 × pitch. Because the removal happens on both sides, the diameter shrinks by twice that: 1.08253 × pitch, which is the metric constant.
The inch constant is the same geometry expressed in threads per inch. Pitch is 1/n, so the diameter reduction is 1.08253 ÷ n. The value normally quoted for unified threads is 1.29904 ÷ n, which comes from the older convention of 0.64952 ÷ n per side — that is 0.75 H rather than 0.625 H, a slightly deeper reference form that has been the basis of published tap drill tables for a century. This calculator uses 1.29904 for inch threads and 1.0825 for metric, which is why the same nominal percentage produces slightly different results in the two systems, and it is also why every published chart agrees with the numbers here.
One consequence is worth memorising. The traditional metric shop rule — drill diameter = major diameter minus pitch — always produces exactly 1 ÷ 1.0825 = 92.4% engagement, no matter what thread you apply it to, because the pitch cancels. It is a fast rule and a heavy one: on an M10 × 1.5 it means an 8.5 mm drill instead of the 8.8 mm a 75% target would call for.
Worked example: 1/4-20 UNC at 75%, and the same hole at 65%
A 1/4-20 UNC thread has a major diameter of 0.2500 in and 20 threads per inch.
- Full thread depth on diameter. 1.29904 ÷ 20 = 0.064952 in.
- Depth removed at 75%. 0.75 × 0.064952 = 0.048714 in.
- Theoretical drill. 0.2500 − 0.048714 = 0.20129 in.
- Nearest standard drill. A #7 drill is 0.2010 in — 0.0003 in under the theoretical size. This is the tap drill every chart lists for 1/4-20.
- Engagement it really gives. (0.2500 − 0.2010) × 20 ÷ 1.29904 × 100 = 0.98 ÷ 1.29904 × 100 = 75.4%.
- Minor diameter for reference. 0.2500 − 0.064952 = 0.18505 in, which is what a 100% thread would need.
Now suppose you are tapping 316 stainless and want to protect the tap. Target 65%: 0.65 × 0.064952 = 0.042219, so the drill is 0.2500 − 0.042219 = 0.20778 in. The nearest standard sizes are a #4 at 0.2090 in, which gives (0.2500 − 0.2090) × 20 ÷ 1.29904 = 63.1%, and a 13/64 in at 0.20313 in, which gives 72.1%. Choose the #4 and you have deliberately traded a few percent of thread for a tap that is much less likely to snap in the hole.
Choosing the engagement, not just accepting 75%
Use 75% as the default for through-tapped steel, aluminium and cast iron where the engagement length is at least one diameter. It is the value the published charts are built on, and it balances torque against strength for ordinary work.
Drop to 55–65% when the tap is small, the material is gummy or work-hardening, or the hole is blind and deep. Austenitic stainless, Inconel, titanium and soft aluminium all reward a bigger drill: the tap sees less material, the chips are thinner, and the torque falls roughly in proportion to the extra engagement you gave away. Broken taps almost always come from torque, and torque is set here.
Go above 80% only when the engagement length is short — thin sheet, a boss you cannot make deeper, a thread in plastic or in a soft casting where the crests carry real load. Even then, check that the tap can survive it, and use a spiral-point tap with through-hole chip ejection where you can.
Whatever you choose, the drill you actually own is what determines the result. Standard drills come in discrete steps, so the achieved engagement rarely equals the target; a step in drill size near 1/4 in changes engagement by roughly ten percentage points. Read the achieved figure rather than the target, and prefer the larger drill when in doubt — a slightly loose thread that taps cleanly beats a broken tap in a nearly finished part.
Tap drill sizes for common unified threads at 75% engagement
| Thread | Major dia (in) | TPI | 75% drill (in) | Standard drill | Its size (in) | Actual engagement |
|---|---|---|---|---|---|---|
| 4-40 UNC | 0.1120 | 40 | 0.0876 | #43 | 0.0890 | 70.8% |
| 6-32 UNC | 0.1380 | 32 | 0.1076 | #36 | 0.1065 | 77.6% |
| 8-32 UNC | 0.1640 | 32 | 0.1336 | #29 | 0.1360 | 69.0% |
| 10-24 UNC | 0.1900 | 24 | 0.1494 | #25 | 0.1495 | 74.8% |
| 10-32 UNF | 0.1900 | 32 | 0.1596 | #21 | 0.1590 | 76.4% |
| 1/4-20 UNC | 0.2500 | 20 | 0.2013 | #7 | 0.2010 | 75.4% |
| 1/4-28 UNF | 0.2500 | 28 | 0.2152 | #3 | 0.2130 | 79.8% |
| 5/16-18 UNC | 0.3125 | 18 | 0.2584 | F | 0.2570 | 76.9% |
| 3/8-16 UNC | 0.3750 | 16 | 0.3141 | 5/16 | 0.3125 | 77.0% |
| 1/2-13 UNC | 0.5000 | 13 | 0.4251 | 27/64 | 0.4219 | 78.2% |
| 5/8-11 UNC | 0.6250 | 11 | 0.5364 | 17/32 | 0.5313 | 79.4% |
Actual engagement scatters from 69% to 80% purely because drill sizes are discrete. That spread is normal and is why published charts differ from each other by a size in places.
Tap drill sizes for coarse metric threads
| Thread | Pitch (mm) | 75% drill (mm) | Nearest drill | Its engagement | “D − pitch” drill |
|---|---|---|---|---|---|
| M3 | 0.50 | 2.594 | 2.6 mm | 73.9% | 2.50 mm |
| M4 | 0.70 | 3.432 | 3.4 mm | 79.2% | 3.30 mm |
| M5 | 0.80 | 4.351 | 4.4 mm | 69.3% | 4.20 mm |
| M6 | 1.00 | 5.188 | 5.2 mm | 73.9% | 5.00 mm |
| M8 | 1.25 | 6.985 | 7.0 mm | 73.9% | 6.75 mm |
| M10 | 1.50 | 8.782 | 8.8 mm | 73.9% | 8.50 mm |
| M12 | 1.75 | 10.579 | 10.6 mm | 73.9% | 10.25 mm |
Most published metric charts list the D − pitch value because it falls on a stocked drill size. It is a heavier thread than inch practice targets, which is one reason metric taps in small sizes have a reputation for breaking.
What this calculation does not cover
- Form taps need a different, larger hole. A roll or form tap displaces material rather than cutting it, so the hole must be sized for the volume of metal that will flow. Use the tap maker's table — a cut-tap drill in a form-tapping operation will break the tap.
- Drills cut oversize. A twist drill typically produces a hole a few thousandths over nominal, which lowers the engagement you actually get. In critical work, measure the hole rather than trusting the drill marking.
- Pipe threads are tapered and follow their own tables. NPT and BSPT tap drills are not derived from a percentage of thread and cannot be computed this way.
- Thread class is not modelled. Classes 2B and 3B differ in tolerance on the pitch diameter, not in the tap drill; the drill sets the minor diameter, and the tap sets the class.
- Very short engagement lengths change the trade-off. In material thinner than about one thread diameter, the internal thread really can be the failing member, so higher engagement earns its torque.
- Chamfering matters. A hole chamfered to slightly over the major diameter guides the tap and prevents a raised burr around the thread; that chamfer removes the first partial thread, which is intended.
Getting from the drilled hole to a working thread
The tap drill is one step in a short chain, and the steps before and after it are worth doing properly. The hole must be drilled at a sensible speed and feed — the drilling speed and feed calculator covers RPM, feed per revolution and the torque a given drill will draw — and it must be deep enough. A blind hole needs the thread depth you want plus the tap's chamfer length plus room for chips: three or four extra pitches is the usual minimum for a plug tap and more for a bottoming operation.
What the thread is for decides how much of this matters. A tapped hole that will carry a bolt to a real preload is a structural joint, and the number that governs it is the tightening torque and the resulting clamp load rather than the thread engagement — the bolt torque calculator works that out from the bolt grade and the nut factor. What tap drill selection contributes to that joint is simply that the internal thread must not be the weak link, which for a steel bolt in steel means an engagement length of about one diameter at any sensible percentage of thread.
Where the hole is a fit rather than a thread, a different standard applies: the ISO hole and shaft fit calculator resolves the limits and clearances for symbols such as H7/g6. The thread geometry used here is defined in ASME B1.1 for unified inch threads and ISO 68-1 for the metric form, with Machinery's Handbook reproducing the tap drill tables that the calculator reproduces from first principles.