A cutting tap wants a hole a little under the screw, not a full-depth V. This calculator is locked at 75% thread — the usual shop compromise between strength and tap torque. Unified inch uses diameter minus 0.974 over TPI. Metric uses diameter minus pitch. The page then names the closest numbered, letter, or fractional drill.
A cutting tap wants a hole a little under the screw, not a full-depth V.
Use it before tapping a hole in steel, aluminium or plastic for an inch or metric thread. It gives the theoretical drill diameter for the common 75% thread rule and the nearest standard drill. Tough materials and deep holes are often drilled a touch larger, which eases tapping and costs little strength.
Percent of thread is how much of the sharp V the tap is asked to cut. 100% is the full theoretical height. It is only a few percent stronger than 75% and takes much more torque — small taps break there. Shop charts and this page sit on 75%.
Unified inch (75%): drill = D − 0.974 / TPI
Metric ISO (shop 75%): drill = D − pitch
The 0.974 inch constant is 75% of the 1.299 height factor on a 60° Unified thread (1.299 × 0.75 = 0.97425, used here as 0.974). Pitch on inch threads is 1/TPI, so a 1/4-20 screw is 0.250 − 0.974/20 = 0.2013 in. Metric ISO uses the even shorter shop rule — subtract the pitch in millimetres. M8 × 1.25 is 8 − 1.25 = 6.75 mm.
That theoretical hole is then matched to a stocked drill. Inch lookup is the closest among numbered bits #80–#1, letter bits A–Z, and fractional bits in 1/64 in steps through 2 in. Closest means smallest absolute difference; an exact distance tie takes the larger drill (a hair less engagement, easier on the tap). Metric lookup is the nearest 0.1 mm jobber size, ties rounding up, so 6.75 mm becomes 6.8 mm.
Cutting taps only. A forming (roll) tap displaces metal and wants a larger hole. This page does not pick a material, a spiral-flute vs spiral-point, or a tap from a catalog.
| Thread | Arithmetic | Theoretical | Closest drill |
|---|---|---|---|
| 1/4-20 UNC | 0.250 − 0.974/20 | 0.2013 in | #7 (0.2010 in) |
| M8 × 1.25 | 8 − 1.25 | 6.75 mm | 6.8 mm |
| #10-24 UNC | 0.190 − 0.974/24 | 0.1494 in | #25 (0.1495 in) |
| #10-32 UNF | 0.190 − 0.974/32 | 0.1596 in | #21 (0.1590 in) |
| 5/16-18 UNC | 0.3125 − 0.974/18 | 0.2584 in | F (0.2570 in) |
| 3/8-16 UNC | 0.375 − 0.974/16 | 0.3141 in | 5/16 in (0.3125 in) |
Those six rows use the 0.974 factor (not 0.9743), the same as the calculator. 1/4-20 is the usual inch check: 0.2013 in lands on a #7. M8 × 1.25 is the usual metric check: 6.75 mm lands on 6.8 mm.
A short chart of the same 75% arithmetic. The calculator above covers these and any custom major/pitch.
| Thread | Major | Pitch / TPI | Closest drill |
|---|---|---|---|
| #4-40 UNC | 0.112 in | 40 TPI | #43 |
| #6-32 UNC | 0.138 in | 32 TPI | #36 |
| #8-32 UNC | 0.164 in | 32 TPI | #29 |
| 1/4-28 UNF | 0.250 in | 28 TPI | #3 |
| 1/2-13 UNC | 0.500 in | 13 TPI | 27/64 in |
| M3 × 0.5 | 3 mm | 0.5 mm | 2.5 mm |
| M4 × 0.7 | 4 mm | 0.7 mm | 3.3 mm |
| M5 × 0.8 | 5 mm | 0.8 mm | 4.2 mm |
| M6 × 1.0 | 6 mm | 1.0 mm | 5.0 mm |
| M10 × 1.5 | 10 mm | 1.5 mm | 8.5 mm |
Percent of thread is a tradeoff: higher percent means a tighter female thread and more tap torque; lower percent taps easier in tough alloys. Many shop charts center near 75% for general work — enter the percent your chart or job calls for.
The formula on this page uses major diameter and thread pitch (or TPI) as shown in the worked checks. Confirm whether you are in inch unified or metric before you drill. A letter/number drill that lands nearest the computed size is normal; the calculator’s nearest-drill note is a convenience, not a guarantee every bit is in your index.
Units: Major diameter and drill size in inches (or mm in metric mode). Pitch in threads per inch or mm/thread as labeled.
Blind holes need depth for chip clearance and tap lead. This calculator sizes the hole diameter, not hole depth or spiral-point vs hand-tap selection.
It is 75% of the sharp-V thread height, not 75% of the screw’s major diameter. The remaining 25% is the gap at the root that a cutting tap never fills. Fastener strength in steel is already close to the bolt’s own strength at about 60–75%. Going past 75% mostly raises tap torque.
Unified and ISO metric are both 60° threads, but the shop formulas are not written the same way. Inch charts fold 75% × 1.299 into 0.974 and divide by TPI. Metric shop practice subtracts the pitch in millimetres, which lands near 75% on coarse ISO pitches. This page uses those two published shop rules, not a third blended constant. A more formal metric 75% would be D − 0.974 × pitch (M8 would be 6.78 mm) and still round to 6.8 mm.
Whichever name the calculator prints. Numbered and letter drills fill the gaps between 1/64 in steps. A #7 is 0.2010 in; 13/64 in is 0.2031 in. They are not interchangeable if you care about the last two thousandths. If your index only has fractions, 13/64 in is the next common size above a #7 — a hair more clearance, a hair less thread.
No. A forming tap pushes metal into the thread instead of cutting chips, so the pre-drill is larger — often close to the pitch diameter, not the 75% cutting size. Use the tap maker’s forming chart. This page will not guess that hole.
Hard, gummy, or work-hardening alloys are often tapped at 60–70% so the tap survives. Soft aluminum can take a higher percent if you want more engagement in a short hole. This calculator stays on 75% and does not shift with material. If the tap maker prints a different drill, that table wins.
Set Common size to Custom. Inch majors accept 0.25, 1/4, 5/16, 1/2, or a machine-screw number like #10 (major = 0.060 + 0.013 × N). TPI is the number after the dash. Metric majors and pitches are millimetres — M12 × 1.75 is 12 and 1.75.