How we calculate

Every number on this site is calculated from the thread standards, then compared with published tap drill charts. A value only goes on a page when at least two independent published sources agree with it. When they do not, we leave it out and say so.

Thread geometry

Unified inch threads (UNC, UNF) follow ASME B1.1; metric threads follow ISO 261 and ISO 262 for sizes and pitches and ISO 965-1 for tolerances. Both use the same 60 degree profile, so the same formulas apply. With major diameter D and pitch P (P = 1 / threads per inch):

• Basic pitch diameter = D − 0.649519 × P
• Basic minor diameter of the nut (internal thread) = D − 1.082532 × P
• Basic thread height of the nut = 0.541266 × P

Percent of thread

The percentage tells you how much of a full-depth thread a drill leaves for the tap to cut:

% thread = (D − drill) ÷ (1.299038 × P) × 100

This is the formula in Machinery's Handbook and in tap makers' charts. 75% is the usual design point: going higher adds little strength but makes the tap much harder to turn, which is how small taps break. Hard or gummy materials are often tapped at 60 to 65%.

Choosing the tap drill

Inch threads: we pick the number, letter or fractional drill closest to 75% thread. That reproduces the drill on the published charts for every UNC and UNF thread from #0-80 to 7/8-14.

Metric threads: the ISO convention is drill = D − P (M8 x 1.25: 8 − 1.25 = 6.75), rounded to a stocked drill. Where D − P falls exactly between two stocked drills we use the size listed in ISO 2306 (10.2 mm for M12 x 1.75, 5.2 mm for M6 x 0.75).

Alternatives shown next to the main drill must give 60 to 80% thread and stay inside the minor diameter limits of the thread class.

Minor diameter limits

Each drill is checked against the tolerance band of the nut's minor diameter: class 2B for inch threads (ASME B1.1 formulas: 0.25P − 0.4P² from 1/4 in up, 0.05P^2/3 + 0.03P/D − 0.002 below) and class 6H for metric (ISO 965-1, tolerance grade 6). A drill outside that band can still make a usable thread, but it is not a standard one.

Clearance holes

Close, normal and loose fits come from ASME B18.2.8 for inch screws and ISO 273 for metric. We publish them only for sizes where two independent reproductions of the standard agree. #2, #4, #12 and 7/16 inch are not covered yet.

NPT pipe threads

Pipe outside diameter, threads per inch and hand-tight engagement L1 come from ASME B1.20.1; the pitch diameters E0 and E1 and the effective thread length L2 are calculated with its formulas (E0 = D − (0.05D + 1.1)P, L2 = (0.8D + 6.8)P). The tap drill is the size for tapping without a taper pipe reamer.

Rules of thumb we label as such

Some advice on the thread pages is shop practice, not a standard, and the page says so: thread engagement of 1 × D in steel and 1.5 to 2 × D in softer metals, drilling 5 pitches deeper than the thread for a plug tap, and the thread-forming tap drill formula D − 0.0068 × 65 ÷ TPI used by tap makers. Check your tap maker's chart before drilling for a forming tap.

Checking against published charts

The current build checks 78 threads, 144 drill diameters and 42 clearance holes. 75 threads match at least two charts; the rest are left out of the thread pages. Sources:

• J.C. Gupta & Sons, Tap Drill Sizes Unified (PDF)
• Lincoln Machine, Tap Drill Chart
• Victor Machinery Exchange, Tap Drill Sizes
• East Tennessee State University, Tap, Drill and Clearance Hole Sizes
• LittleMachineShop.com, Tap and Clearance Drill Sizes (PDF)
• American Fastener Technologies, Tap and Drill Size Chart
• Wikipedia: List of drill and tap sizes, Drill bit sizes, National pipe thread
• Engineers Edge: internal thread tables (ASME B1.1, ASME B1.13M) and NPT dimensions (ASME B1.20.1)
• isocnc.com, calcformula.com, PI Fabricators and Grokipedia for ASME B18.2.8 and ISO 273 clearance holes

Where the charts disagree

Published charts are not all the same, and the differences are systematic rather than random:

• Victor Machinery's chart lists one number size smaller for several small screws (#51 for 2-56, #17 for 12-24). Those drills cut about 80% thread instead of 70 to 75%.
• Lincoln Machine's metric column, which Wikipedia shares, uses drills 0.1 to 0.3 mm larger than D − P (6.9 mm for M8 x 1.25, 10.5 mm for M12 x 1.75), about 66 to 68% thread. Because the two match each other, we do not count them as independent sources.
• For 1-12 UNF, M12 x 1.25 and M18 x 1.5 we have only one matching source so far, so those threads have no page yet.

Found a number you think is wrong? Tell us through the contact page with the source you are comparing against.