Tap Drill Size Chart

How these numbers are calculated

Thread engagement is set by how much smaller the hole is than the thread's major diameter. Both formulas below come from the basic 60° thread form, so the whole table is reproducible — you can check any row by hand.

Inch:    drill = D − 0.0130 × %thread × (1 / TPI)
Metric:  drill = D − (%thread / 76.8) × pitch

The metric formula is written against 76.8 rather than 100 for a reason: at exactly 76.8% it reduces to drill = D − pitch, which is the rule most machinists already carry in their head. That is why M6×1.0 gets a 5.0 mm drill and not the 5.02 mm that a literal 75% would ask for.

Why the "Actual %" column matters

Drills come in fixed sizes, so you almost never hit the engagement you asked for. Ask for 75% on a 1/2-13 and the nearest drill (27/64″) actually delivers 78.1% — a stiffer tap, more torque, more heat. Ask for 75% on a 1/4-20 and a #7 gives you 75.4%, which is close enough to ignore.

Charts that only print the drill size hide this. Knowing the real number tells you when to expect a hard tap and when you have room to go one size up in tough material.

When the drill set cannot hit the number

Fine threads step engagement faster than the 1/64″ drill set steps diameter, so on some sizes no available drill lands near the figure you asked for. A 1/2-20 at a nominal 85% actually gives 96% with the nearest drill — far tighter than intended. Those rows carry a ! in the table. Where it matters, a metric drill often lands closer: the same 1/2-20 takes 11.3 mm for a true 85%.

Choosing an engagement percentage

• 50–60% — hard or gummy material, deep holes, hand tapping. Much lower breakage risk.
• 75% — the default for steel and aluminum in most shops.
• 85%+ — thin material or soft alloys where you need every bit of thread you can get. Expect heavy torque.

Going from 75% to 50% engagement costs far less strength than it sounds like, while cutting tapping torque substantially — which is why 50% is common in production work. Verify the exact strength trade-off against your own joint requirement rather than treating a rule of thumb as a spec.

Clearance holes

The last column is a normal-fit clearance hole — the size to drill in the part that the fastener passes through, not the part being tapped. Confusing the two is the most common mistake with these charts.

Related charts

• Drill bit size chart — all four size systems side by side, with equivalence groups
• Thread size chart — pitch diameter, minor diameter and tensile stress area