Percent of Thread Explained: Why Tap Drill Charts Use 75%
What percent of thread means, why charts target about 75%, how strength and tapping torque trade off, and how to pick a drill for your material.
- percent of thread
- tap drill basics
- thread strength
- tapping torque
- materials
Quick answer: Percent of thread is how tall the tapped thread is compared with a full, theoretical thread. Tap drill charts aim for about 75% because it gives nearly all the useful strength while keeping tapping torque reasonable. Going higher adds very little strength and a lot of torque. Going lower, to about 60–65%, makes tapping much easier and is the usual choice for stainless steel and other tough metals. For a 1/4-20, the chart drill is a #7 (0.201 in) at 75.4%, and the lower-thread option is a #3 (0.213 in) at 57%.
What percent of thread actually measures
Every thread has a basic minor diameter: the smallest hole that would still let a full-height thread form. For a 1/4-20 that internal minor diameter is 0.1959 in. If you drilled exactly that size, the tap would cut 100% of the thread height.
Nobody does that. Instead you drill a little bigger, so the tap cuts shorter teeth. The ratio of the height you actually get to the full height is the percent of thread.
The formulas we use on every page on this site:
- Inch threads: % thread = 76.98 × TPI × (major diameter − drill diameter)
- Metric threads: % thread = (major diameter − drill diameter) ÷ (0.01299 × pitch)
Run the 1/4-20 with a #7 drill: 76.98 × 20 × (0.250 − 0.201) = 75.4%. For the full derivation, see our tap drill formula guide.
Why the charts settle on 75%
There are two forces pulling in opposite directions.
Strength goes up as the thread gets taller, but not in a straight line. A shorter thread still has most of its cross-section at the root, where the load sits. OSG’s tapping guide illustrates this: a 60% thread keeps about 73% of the thread’s cross-sectional area, not 60%.
Tapping torque climbs fast as the hole gets smaller, because the tap removes more metal at the root. OSG’s torque test on an M10 tap shows torque rising steeply as thread percentage moves from about 74% toward 98%, up to the point of breaking the tap.
Tap makers put numbers on the trade-off:
- Guhring says a 100% thread is only about 5% stronger than a 75% thread but needs about three times the torque.
- Komet (writing in Canadian Metalworking) gives the same 5% figure and calls 65–70% the sweet spot for cutting taps.
- Tapmatic says strength stops increasing at roughly 75%, while torque “rises exponentially” beyond it.
So 75% became the chart standard. It sits close to the top of the strength curve without paying the torque penalty of a fuller thread. Thread length matters too: a short engagement can strip even at 75%, so percent of thread is only half of the strength story.
Where strength stops paying off
Sources differ on exactly where the curve flattens. Tapmatic puts the knee at about 75%. Guhring recommends 60–70% for most applications. Komet says 65–70%. Tapmatic adds that in tough materials such as stainless steel and Monel, threads as low as 50% can still do the job.
The practical reading: above roughly 60–65%, each extra percent of thread buys little strength and costs more torque and more broken taps. That’s why many machinists drill one size over the chart in steel, and two sizes over in stainless.
One thread, several drill choices
Here’s how the common drill sizes work out for a 1/4-20 (major diameter 0.250 in), using the formula above:
| Drill | Diameter (in) | % thread |
|---|---|---|
| #8 | 0.199 | 78.5% |
| #7 (chart) | 0.201 | 75.4% |
| #6 | 0.204 | 70.8% |
| #5 | 0.2055 | 68.5% |
| #4 | 0.209 | 63.1% |
| #3 | 0.213 | 57.0% |
Every one of those will make a usable thread. The difference is how hard the tap works. Our 1/4-20 page lists the #7 as standard and the #3 as the hard-material option.
Metric works the same way. An M8 x 1.25 uses a 6.8 mm drill for 73.9%. Step up to 7.0 mm and you’re at 61.6%. An M6 goes from 5.0 mm (77.0%) to 5.2 mm (61.6%).
Fine threads run a higher percentage
Fine threads have shallower teeth, so a few thousandths of drill size swing the percentage more. A 1/4-28 on its chart drill, a #3, comes out at 79.8%. The next size up, a #2, gives 62.5%. With fine threads, it’s worth checking the actual percentage instead of assuming the chart drill is near 75%.
Large coarse threads too
On a 1-8 UNC, the chart drill is 7/8 in, which gives 77.0%. Komet points out that modern drills cut very close to nominal size, so a 7/8 drill really does produce close to 77%, which is higher than most applications need. For big taps turned by hand, a slightly larger drill can make the difference between finishing the hole and breaking the tap.
How to pick percent of thread by material
Use this as a starting point, based on Tapmatic’s published ranges and Guhring’s general advice:
| Material | Average work | Deep holes | Thin sheet |
|---|---|---|---|
| Stainless steel, Monel, nickel steel, drop forgings | 60–70% | 55–65% | n/a |
| Aluminum, brass, bronze, cast iron, copper, mild steel | 65–75% | 60–70% | 75–85% |
A few rules of thumb come out of this:
- Tough or work-hardening metals get less thread. Stainless steel is the classic case. See our stainless tapping guide.
- Soft metals and thin material get more. In aluminum or sheet stock, the standard 75% drill is a sensible default, and thin sheet may justify more. See tapping aluminum.
- Deep holes get less. More thread length means more friction and more chips. Dropping the percentage helps.
- Plastics have their own rules. See tapping plastic.
When not to go lower
Lower percent of thread isn’t free. Check these before drilling oversize:
- The drawing. If a print calls out a minor diameter or thread class, the drill has to land inside that limit.
- Short engagement. If the thread is only a couple of turns long, such as in thin sheet, you need every bit of height you can get.
- Form taps. Thread forming taps work completely differently and use larger holes on purpose. Use our form tap drill chart and see cut vs. form tapping.
The short version
Use the chart drill (about 75%) when you don’t know any better. Step up one or two sizes, toward 60–65%, when the material is tough, the hole is deep, or the tap keeps breaking. Stay at 75% or slightly above in soft metals and thin stock. Every thread page on this site shows the standard drill and a 60% drill side by side, and the UNC tap drill chart and metric tap drill chart list the percentage for each.
Sources: Guhring Tap Drill Calculator notes (guhring.com/tech/TapDrill); Tapmatic, “Tapping Torque vs. Thread Strength” (tapmatic.com); OSG Tap Technical Guide Vol. 1, sections 8.2 and Fig. 30–31; Cullen Morrison (Komet), “Common issues with thread tapping,” Canadian Metalworking, 2014.