Tap Drill Formula Explained, With Worked Examples

Quick answer: For inch threads, drill = major − (0.01299 × % thread ÷ TPI). For metric threads, drill ≈ major − pitch (about 77% thread). For form taps, swap 0.01299 for 0.0068. Then pick the nearest drill you actually own and check its real percent of thread with % = 76.98 × TPI × (major − drill). Example: 1/4-20 at 75% works out to 0.2013 in, so a #7 drill (0.201 in) gives 75.4%.

Tap drill charts are handy, but knowing the formula lets you check a chart, work out an odd size, or decide whether the drill in your hand is close enough. Here is how it works, with real numbers.

The inch formula (cut taps)

Inch threads are named by major diameter and threads per inch (TPI). Pitch is just the inverse: pitch = 1 ÷ TPI. A 1/4-20 has a 0.250 in major diameter and a 0.050 in pitch.

The drill formula is:

Drill = Major − 0.01299 × % thread × pitch

You can also write it as major − (0.01299 × %) ÷ TPI. Tap makers and suppliers publish it in this form, including Tapmatic’s tapping formulas. Enter the percent as a whole number: 75, not 0.75.

The reverse formula tells you what thread you get from a drill you already have:

% thread = 76.98 × TPI × (Major − Drill)

The two constants are linked: 1 ÷ 0.01299 = 76.98.

Worked example: 1/4-20 at 75%

1. Pitch = 1 ÷ 20 = 0.050 in
2. 0.01299 × 75 × 0.050 = 0.0487 in
3. Drill = 0.250 − 0.0487 = 0.2013 in

No drill is exactly 0.2013 in, so look at the neighbors:

The #7 is the closest and lands right on target, which is why it is the standard 1/4-20 tap drill. If you only have fractional drills, 13/64” is a reasonable stand-in at 72.2%.

Worked example: 5/16-18 at 75%

1. Pitch = 1 ÷ 18 = 0.05556 in
2. 0.01299 × 75 × 0.05556 = 0.0541 in
3. Drill = 0.3125 − 0.0541 = 0.2584 in

The nearest drills are F (0.257 in, 76.9%) and G (0.261 in, 71.4%). F is the chart answer for 5/16-18.

Worked example: a lower percent for tough material

Say you are tapping 1/4-20 in something hard and want about 60% thread:

0.250 − (0.01299 × 60 × 0.050) = 0.250 − 0.0390 = 0.2110 in

That falls between a #4 (0.209 in, 63.1%) and a #3 (0.213 in, 57.0%). Our charts list the #3 as the 60% “hard material” drill for 1/4-20. Either is defensible; the #3 is easier on the tap.

Why would you give up thread depth on purpose? Guhring, the tap maker, notes that most charts target about 75%, suggests 60% to 70% for most applications, and says a 100% thread is only about 5% stronger than 75% while taking about three times the torque to produce (Guhring tap drill calculator). Our percent of thread guide goes deeper on this trade-off.

What “100% thread” means here

The 0.01299 constant comes from treating 1.299 × pitch as the full double thread depth. That makes a “100%” hole the same size as the minor diameter of the external thread, as given in Machinery’s Handbook (MechaniCalc thread equations). The basic internal minor diameter is smaller still: major − 1.0825 × pitch, which works out to about 83% on this scale.

For 1/4-20, the basic internal minor diameter is 0.1959 in. The 75% drill (0.2013 in) is a little larger, which is normal: chart drills deliberately leave a slightly shallower thread so the tap cuts less metal.

The metric quick rule

Metric threads are named by major diameter and pitch in millimeters, like M8 x 1.25. The shortcut is:

Drill ≈ Major − Pitch

Because 1 ÷ 0.01299 = 76.98, “major minus pitch” always gives about 77% thread, whatever the size. That is why the rule is so popular.

M8 is the odd one out. There is no common 6.75 mm drill, so charts use 6.8 mm, which gives about 74%.

If you want a specific percent in metric, use the same formula as inch, all in millimeters:

Drill (mm) = Major − 0.01299 × % × Pitch % thread = (Major − Drill) ÷ (0.01299 × Pitch)

Check M8 x 1.25 with a 6.8 mm drill: (8 − 6.8) ÷ (0.01299 × 1.25) = 1.2 ÷ 0.01624 = 73.9%. Tapmatic publishes the same relationship using 76.98 as the divisor.

Form tap formula

Form taps (also called roll taps or thread-forming taps) do not cut chips. They push metal into the thread shape, so the hole must start larger. The formula keeps the same shape with a smaller constant:

Form tap drill = Major − 0.0068 × % × pitch

Most form tap charts aim for about 65%.

1/4-20 at 65%: 0.250 − (0.0068 × 65 × 0.050) = 0.250 − 0.0221 = 0.2279 in, so use a #1 drill (0.228 in).

M8 x 1.25 at 65%: 8 − (0.0068 × 65 × 1.25) = 8 − 0.5525 = 7.447 mm, so use a 7.4 mm drill.

Both match the published worked examples in KAR Industrial’s forming tap reference, which writes the metric version as % × pitch ÷ 147.06 (1 ÷ 0.0068 ≈ 147). Treat the result as a starting point. Form tapping is sensitive to hole size, and tap makers’ own charts can differ by a few thousandths, so check the maker’s recommendation for your tap. See the form tap drill chart and our guide to cut vs form tapping.

How to pick the nearest real drill

The formula gives a theoretical number. Your drill index gives you a short list of real sizes. Standard US sets cover number drills (#80 to #1), letter drills (A to Z), fractional drills in 1/64” steps, and metric drills. Here is a simple process:

1. Calculate the theoretical drill for your target percent.
2. List the closest drill above and below it from the sets you own.
3. Run the percent formula on each to see what you actually get.
4. Choose by material and depth:
   • Hard, tough or gummy materials, deep holes, and small taps: lean toward the larger drill (lower percent, less torque, fewer broken taps).
   • Soft materials, thin walls, or when you need every bit of grip: the smaller drill is fine, but every percent above 75 adds torque for very little extra strength.
5. Remember the drill cuts oversize. Guhring notes that actual percent of thread varies from the target because of drilling runout. A worn or wobbly drill makes a bigger hole and a shallower thread.

A quick cross-check: for 1/4-20, a metric 5.1 mm drill (0.2008 in) gives 75.7%, almost identical to the #7. Mixing inch and metric drills is perfectly fine as long as you run the numbers.

Quick reference

For the finished answers, use the UNC tap drill chart, UNF chart or metric chart. For the screw that passes through the mating part, see the clearance hole chart.