Why no two tap drill charts agree
Thread engagement percentage sounds like a physical measurement and it is not. It is a ratio, and the denominator is a matter of convention. The numerator is easy: how much smaller than the major diameter your hole is, halved, because the thread cuts in from both sides. The denominator is the depth at which the thread would be considered complete, and there are two references in common use.
The first is 1.0825 times the pitch. That is the distance from the major diameter down to the basic minor diameter of the internal thread as defined in ASME B1.1 and ISO 68, arrived at by truncating the sharp fundamental triangle at five eighths of its height on each side. It is the number the standards use, and it is what this page defaults to.
The second is 1.299 times the pitch, which measures to a deeper reference. Very many published shop charts, and most of the pocket cards handed out with tap sets, are computed on this basis. The consequence is that the same physical hole reads about 75 percent on one convention and about 90 percent on the other. Neither chart is lying and neither drill is wrong. They are two labels for the same piece of metal.
The concrete case: 1/4-20 UNC. On the 1.0825 basis, a 75 percent hole is 0.250 minus 0.75 times 0.0541, which is 0.2094 inches, and the nearest standard drill is a #4 at 0.209. The chart on the wall says #7 at 0.201, and calls it 75 percent. Put #7 through the 1.0825 formula and it comes out at 90.5 percent. This is exactly why the percentage is an input on this page rather than baked in. Decide what you want, know which convention you are quoting it in, and the drill follows.
What engagement percentage actually buys you
Very little, past a point, and this is the most useful thing on the page. A tapped joint fails by stripping the threads along the whole engaged length, not by shearing off the tip of one thread. Increasing depth of engagement from 60 percent to 100 percent adds roughly 5 percent to the stripping strength while roughly doubling the torque required to cut it. That is a terrible trade, and it is the reason experienced people drill loose and sleep well.
| Engagement | Where it makes sense |
|---|---|
| 55-65% | Deep holes, tough material, hand tapping, anywhere a broken tap would be expensive to remove |
| 65-75% | General shop work. This is the sweet spot for almost everything. |
| 75-85% | Thin material where you cannot get enough engaged length, soft alloys, aluminium bosses |
| Above 85% | Rarely justified. Torque climbs steeply, strength does not. |
Engaged length is the lever that actually matters. A rule that holds up well: engage at least one diameter of thread in steel, one and a half in cast iron or brass, and two in aluminium or plastic. A 1/4-20 in aluminium wants half an inch of thread. Getting that right will do more for the joint than any amount of fussing over whether the hole is 0.201 or 0.209.
Metric charts are simpler than they look
Nearly every metric tap drill chart in existence uses one rule: hole equals major diameter minus pitch. M6 x 1 gets a 5.0 mm drill. M8 x 1.25 gets 6.8, which is 8 minus 1.25 rounded to a stock drill. M10 x 1.5 gets 8.5. That rule corresponds to about 92 percent engagement on the 1.0825 basis, which is deeper than most shops actually want, and it is why metric taps in aluminium have a reputation for being grabby. Going one drill size up from the chart, to 5.2 for M6 or 7.0 for M8, drops you to something nearer 75 percent and makes the tap noticeably happier.
Clearance holes, and the fits nobody defines out loud
The clearance figures here are computed as proportional offsets and then snapped up to the nearest standard drill. Close fit is roughly one sixty-fourth over the screw for imperial sizes a quarter inch and up, normal is a thirty-second, loose is a sixteenth. For metric the ratios are about 5, 10 and 20 percent over the major diameter, which lands on the ISO 273 fine, medium and coarse series almost exactly for common sizes.
Which one you want is a question about alignment, not strength. Close fit assumes both parts were located accurately and you want the fastener to help hold position. Normal fit is the default for anything assembled by hand from parts made on separate days. Loose fit is for weldments, long bolt patterns, and anything where thermal movement or accumulated tolerance means the holes will not line up. For a bolted structural connection the hole size is specified by the governing code and is not yours to choose.
When the calculator and the chart disagree
Use the drill you have. The gap between a #7 and a #4 in a 1/4-20 hole is the difference between 90 percent and 75 percent engagement, and both make a joint that will strip the bolt before it strips the thread if the engaged length is adequate. What matters far more than the drill number is that the hole is perpendicular, that it is deep enough for the tap to clear, that you used cutting fluid appropriate to the material, and that you backed the tap off to break the chip rather than driving it in until something gave. Nobody has ever had a bracket fail because they picked the wrong side of a tap drill chart.
Questions people ask
What size drill for a 1/4-20 tap?
The traditional answer is a #7 at 0.201 inches, and it is a perfectly good answer. On the ASME definition of engagement that hole gives about 90 percent, which is more thread than you need and more tapping torque than you want. If you would rather tap at around 75 percent, a #4 at 0.209 or a 13/64 at 0.2031 will both serve, and the resulting joint will be within a few percent of the same strength. In steel with a full diameter of engaged thread, any of the three will strip the bolt first.
What drill for an M6 tap?
The chart answer is 5.0 mm, which is simply the major diameter minus the pitch and works out to roughly 92 percent engagement. That is on the tight side, particularly in stainless or aluminium. A 5.2 mm drill drops it to about 75 percent and makes tapping considerably easier for a loss of strength you would struggle to measure. For M6 x 0.75 fine thread the chart says 5.25 mm. Whichever you pick, get at least 6 mm of engaged thread in steel and 12 mm in aluminium.
Why did my tap break?
Most commonly, too much engagement in tough material, or a hole that bottomed out before the tap did. Other regulars: no cutting fluid, a bottoming tap used to start the thread instead of a taper tap, chips packing in a blind hole because nobody backed it off, the tap not square to the hole so it loaded one side, and running a form tap into a hole drilled for a cut tap. Drilling one size larger than the chart is the cheapest single change you can make, and the strength cost is a few percent.
Do form taps use the same drill size?
No, and this is the mistake that snaps them. Roll form taps displace material rather than cut it, so they need a substantially larger starting hole than a cut tap for the same finished thread, typically several thousandths bigger on small sizes and correspondingly more on large. The manufacturer publishes the sizes for their taps and those are the only ones to use. Form taps produce a stronger thread with a burnished surface and no chips, which makes them excellent in ductile material and useless in cast iron.
Can I use a metric drill for an imperial tap or the other way round?
Yes, as long as the diameter is right, and it often is. Metric drills come in 0.05 and 0.1 mm steps, which is finer than number and letter drills over most of the range, so a metric set will usually get you closer to any target than a fractional set will. The calculator here works within one system at a time, but the theoretical diameter it reports is just a number: convert it and pick whatever drill in whatever set lands nearest. A 5.2 mm drill is 0.2047 inches, which sits neatly between a #6 and a #5 and is a fine tap drill for 1/4-20 at around 84 percent.