How the Tap Drill Numbers Are Calculated
Every number on this site is either copied from a published chart and cross-checked, or computed from a stated formula. Nothing is estimated by feel.
Chart drills (the 75% row)
The inch chart drills match two independent published charts: the American Fastener tap and drill chart and the Fabworks tap drill chart. Drill diameters come from Wikipedia: drill bit sizes. Metric chart drills are the major diameter minus the pitch, checked against the Fabworks metric column where it has a clean row.
Thread data
Pitches and threads per inch come from Wikipedia: ISO metric screw thread and Wikipedia: Unified Thread Standard. Numbered screw major diameters follow 0.060 + 0.013 x size.
Thread engagement
Engagement = (major diameter - drill diameter) / (1.299 x pitch). Full thread depth is 0.6495 x pitch per side, so a 100% thread needs a hole of major - 1.299 x pitch. The pitch and minor diameters shown on each page use the basic profile formulas D - 0.649519 x P and D - 1.082532 x P.
The same formula is printed in the OSG tap drill chart, Vol 3 (2024): drill size = major diameter - 0.01299 x percent of full thread / threads per inch. We checked it against the table in that chart. For all 28 inch threads on this site, the hole diameters we compute at 80, 75, 70, 65 and 60% thread match the printed values to within 0.0001 in. The check runs in tests/data.test.mjs every time the site is built.
Here is that check, thread by thread. Both columns are the hole diameter for a 75% thread:
| Thread | Our hole (in) | OSG hole (in) | Difference (in) |
|---|---|---|---|
| #0-80 | 0.0478 | 0.0478 | 0.0000 |
| #2-56 | 0.0686 | 0.0686 | 0.0000 |
| #4-40 | 0.0876 | 0.0876 | 0.0000 |
| #5-40 | 0.1006 | 0.1006 | 0.0000 |
| #6-32 | 0.1076 | 0.1076 | 0.0000 |
| #6-40 | 0.1136 | 0.1136 | 0.0000 |
| #8-32 | 0.1336 | 0.1336 | 0.0000 |
| #10-24 | 0.1494 | 0.1494 | 0.0000 |
| #10-32 | 0.1596 | 0.1596 | 0.0000 |
| #12-24 | 0.1754 | 0.1754 | 0.0000 |
| 1/4-20 | 0.2013 | 0.2013 | 0.0000 |
| 5/16-18 | 0.2584 | 0.2584 | 0.0000 |
| 3/8-16 | 0.3141 | 0.3141 | 0.0000 |
| 7/16-14 | 0.3679 | 0.3679 | 0.0000 |
| 1/2-13 | 0.4251 | 0.4251 | 0.0000 |
| 9/16-12 | 0.4813 | 0.4813 | 0.0000 |
| 5/8-11 | 0.5364 | 0.5364 | 0.0000 |
| 3/4-10 | 0.6526 | 0.6526 | 0.0000 |
| 7/8-9 | 0.7667 | 0.7668 | 0.0001 |
| 1/4-28 | 0.2152 | 0.2152 | 0.0000 |
| 5/16-24 | 0.2719 | 0.2719 | 0.0000 |
| 3/8-24 | 0.3344 | 0.3344 | 0.0000 |
| 7/16-20 | 0.3888 | 0.3888 | 0.0000 |
| 1/2-20 | 0.4513 | 0.4513 | 0.0000 |
| 9/16-18 | 0.5084 | 0.5084 | 0.0000 |
| 5/8-18 | 0.5709 | 0.5709 | 0.0000 |
| 3/4-16 | 0.6891 | 0.6891 | 0.0000 |
| 7/8-14 | 0.8054 | 0.8054 | 0.0000 |
Drills by material
Texas Metalworks tap drill guide suggests 70 to 75% for soft aluminum and brass, 60 to 65% for mild steel, and 50% for stainless, titanium and hardened material. It also says going from 75% to 60% costs only about 5% of pull-out strength. ToolGrit engagement guide says the standard chart targets roughly 75%, which is fine for through holes in mild steel, and that about 90% of thread shear strength is developed at 60% engagement. It suggests 50 to 55% for blind holes in stainless, titanium and hardened steel. The OSG tap drill chart, Vol 3 (2024) says a thread of 55 to 65% is enough for most requirements.
The guides do not agree everywhere:
| Material | Texas Metalworks | ToolGrit | OSG (tap maker) |
|---|---|---|---|
| Aluminum | 70-75% | 60-65% | 65-70% |
| Brass | 70-75% | 70-75% | 65-70% |
| Plastic | not covered | 70-75% | not covered |
| Mild steel | 60-65% | 60-65% | 65-70% |
| Stainless steel | 50% | 55-60% | 60-70% |
| Titanium | 50% | 50-55% | not covered |
Both guides put mild steel at 60 to 65%, while OSG gives 65 to 70% for average work. ToolGrit is lower than Texas Metalworks for aluminum and higher for stainless. OSG asks for more thread in stainless than either guide: 60 to 70% for average work and 55 to 65% for deep holes. OSG also says a 55 to 65% thread is sufficient for most requirements, and that a higher percentage may be needed to meet the minor diameter limits of the thread class specified. Our stainless column follows the lowest target, 50%, so for average work in stainless the steel column is closer to the tap maker's range.
The 60% and 50% rows apply those targets to the real list of standard drills (fractional, number, letter and 0.1 mm metric). Each shows the largest drill that still leaves at least 2 points under the target. Drill sizes come in steps, so when that drill leaves more than 7 points over the target and another drill lands within 5 points under it, we show the second one. When no drill lands close, the page says so and shows the closest.
Fine-pitch metric sizes
The fine-pitch drills on the metric chart are the major diameter minus the pitch, rounded to the nearest 0.1 mm with ties going to the larger drill. We found no published chart for them, so treat them as computed values, and check the percentage next to each.
Sizes beyond the charts we read
The published charts we read stop at M20. M22, M24 and M30 use the major-minus-pitch rule, and their pages say so.
What this does not cover
These are drills for cutting taps in nominal thread sizes. Forming (roll) taps use different drill sizes, and pipe threads such as NPT are tapered. Neither is covered yet. Always check your tap manufacturer's chart before cutting expensive material.
Found a wrong number?
Use the Contact link in the footer or email contact@tapdrillsize.com with the thread and the figure. Corrections are checked against the sources above and fixed on the page, and the page's last reviewed date changes.
Last reviewed October 7, 2026.