Before a tap can cut an internal thread, the hole must leave exactly the right amount of material for the thread flanks — that hole is the tap drill size. Machinery’s Handbook expresses it through the percentage of full thread engagement: drill = major − 1.29904 × pitch × (% ÷ 100), where 1.29904 is (3/4)√3, the engagement factor of the 60° thread form. Published charts are built on 75% engagement for a reason the handbook’s tests make blunt: beyond about 75%, extra engagement adds very little joint strength while the torque to drive the tap rises steeply — a 100% thread is only marginally stronger but several times harder to tap and far more likely to snap the tap in the hole.
The familiar chart answers drop straight out. M10×1.5 at 75% wants a theoretical 8.539 mm; the nearest standard drill is 8.5 mm, which back-computes to 76.98% engagement — revealing the shop rule “metric tap drill = major minus pitch” as this formula at exactly 76.98%. On the inch side, the nearest-drill search runs the fractional, number (#80–#1), and letter (A–Z) gauge tables of ANSI/ASME B94.11M, and a 10.8 mm drill is sometimes closer to the 1/2-13 theoretical size than any inch drill in the box.
Engagement is a dial, not a constant: drop toward 60–65% for stainless, tool steel, titanium, small fragile taps, and deep holes where chip packing multiplies torque — and when more joint strength is needed in soft material, add thread depth (length of engagement of at least the nominal diameter), not thread percentage. The formulas serve cut taps; form (roll) taps displace material rather than removing it, so their drills run roughly halfway between the cut-tap size and the major diameter, and the tap maker’s recommendation wins.