Tap drill sizes for metric threads

The hole decides more about a tapped thread than the tap does. Too small, and the tap has to cut more material, which raises the torque and with it the risk of breaking the tap. Too large, and the thread is shallow. The right drill is easy to find, and the rule behind it explains every value in the tables.

The rule: d − P

For a cutting tap, the drill diameter is the nominal diameter minus the pitch:

$$D_{\text{drill}} \approx d - P$$

M10 has a pitch of 1.5 mm, so the drill is 8.5 mm; M6 × 1 takes 5.0 mm; M20 × 1.5 takes 18.5 mm. The rule appears in ISO 2306, in DIN 336 and in tool makers’ tables. DIN 336 and the makers’ tables round the result to a standard drill size; for the coarse series only two values differ from d − P:

For M8, d − P would be 6.75 mm; for M12, 10.25 mm. The fine series is rounded the same way: Gühring’s DIN 336 table gives 8.8 mm for M10 × 1.25 and 10.8 mm for M12 × 1.25, where d − P would be 8.75 and 10.75 mm. The full table from M1 to M64, with fine threads, is in the tap drill calculator.

Why d − P works: the 6H limits

The drill makes the minor diameter D1 of the nut thread. ISO 965 gives D1 a tolerance: for the usual class 6H, D1 may lie between its basic value and the basic value plus a tolerance that depends only on the pitch.

Every standard drill falls inside the limits, between 28 % and 58 % of the way from D1 min to D1 max; most sit below the middle of the band. ISO 2306 states the principle behind the choice: within the minor-diameter tolerance, the larger the drilled hole, the more economical tapping becomes. A larger hole leaves less material for the tap to cut, which lowers the cutting torque.

Forming taps need a larger hole

A forming (roll) tap does not cut. It displaces the material, which flows into the crests of the thread, so the hole must be larger. DIN 336 explicitly does not cover cold-forming taps, and published recommendations differ:

The Hommel Hercules document prints its table under the heading “Gewindeschneiden” (thread cutting), but the values are holes for forming taps: all of them lie well above the 6H maximum, which a cutting tap could not use.

OSG uses a formula that also depends on the desired thread percentage and the tap’s tolerance class; for M10 at 90 % it gives 9.24 mm. The sources agree on roughly d − 0.45 P to d − 0.51 P. Use the value of the maker whose tap you use, and measure the minor diameter of the first formed thread.

cut away as chipspressed inmaterial that flows in6H band of D₁basic profile

Thread percentage

“Thread percentage” compares the actual thread overlap with a full thread, but sources use two different definitions of 100 %:

• OSG’s metric guide takes the basic overlap 5H/8. On that basis a d − P hole gives about 92 %.
• OSG’s inch formula takes 3H/4. On that basis the same hole gives about 77 %.

OSG’s tapping guide states that 55 % to 65 % thread is sufficient for most requirements. Before comparing percentages from two tables, check which definition each uses.

OSG metric: 100 % = 5H/8

92 %

P/2 ÷ 5H/8 = 0.750 ÷ 0.812

OSG inch: 100 % = 3H/4

77 %

P/2 ÷ 3H/4 = 0.750 ÷ 0.974

Tapping speed

OSG’s technical guide gives these cutting speeds for its taps, in m/min. Coated taps can run 30 to 50 % faster.

These are one maker’s values for its own taps. The spindle speed follows from n = 1000 · vc / (π · d), and the feed per revolution of a tap is always the pitch.

Hand and spiral fluteSpiral pointForming

For the thread geometry behind these numbers, see ISO metric screw threads.