Tap Drill Size & Thread Calculator
The right drill for any tap, the thread it gives and the nearest stock drills.
Stock drills near the exact size
| Drill | mm | inch | Thread | 6H |
|---|
Thread dimensions
ISO 273 clearance holes for the bolt
How it was calculated
Tap drill chart
About the Tap Drill Size & Thread Calculator
Pick a thread — ISO metric coarse or fine, UNC, UNF, BSP parallel (G) or taper (Rc), NPT, or any metric or unified size you type in — and the calculator gives the usual tap drill and the percentage of thread it produces. It also works out the exact drill for the thread percentage you want and lists the nearest metric and inch (number, letter and fractional) drills with the thread each one gives.
For screw threads it shows the basic major, pitch and minor diameters, the 6H minor-diameter limits for metric threads, the tensile stress area and the ISO 273 fine, medium and coarse clearance holes for the matching bolt. Pipe threads get their gauge-plane diameters, taper and hand-tight engagement. A chart lists every size of the series.
How to use it
- Choose the thread series and the size, or Other metric / Other unified to type a diameter with its pitch or threads per inch.
- Choose cutting tap or forming tap and the thread percentage you want — 75% is usual for cut threads, about 65% for formed ones.
- Read the usual tap drill and its thread percentage, then the stock drills either side of the exact size. Metric results show whether each drill stays inside the 6H minor-diameter tolerance.
- Check the basic dimensions and the clearance holes for the bolt that goes through the mating part.
- Copy result copies the drill, dimensions and clearance holes as text.
Examples
Cutting tap, 75% thread
Usual drill 8.5 mm = 77% thread (6H minor diameter 8.376–8.676 mm). Exactly 75% needs 8.54 mm; clearance holes 10.5 / 11 / 12 mm
Cutting tap, 75% thread
#7 drill (0.201″) gives 75.4% thread; 13/64″ gives 72%
65% thread
Hole = 6 − 0.0068 × 1 × 65 = 5.56 mm; a 5.6 mm drill gives (6 − 5.6) ÷ (0.0068 × 1) = 59% and a 7/32″ drill (5.556 mm) 65%
G 1/2 and 1/2″ NPT
G 1/2: 19 mm drill (minor diameter 18.632–19.173 mm) · 1/2 NPT: 23/32″ drill
The formulas
- Basic profile (ISO 68-1, ASME B1.1): H = 0.866 × P; pitch diameter d2 = d − 0.6495 P; internal minor diameter D1 = d − 1.0825 P; external minor diameter d3 = d − 1.2269 P
- Percentage of thread (Machinery’s Handbook): % = 76.98 × (d − drill) ÷ P, with all sizes in one unit; for inch threads P = 1 ÷ TPI
- Drill for a target percentage: drill = d − % × P ÷ 76.98
- Forming taps (tap makers’ rule): hole = d − 0.0068 × P × %, so a given hole forms % = (d − hole) ÷ (0.0068 × P)
- Quick metric rule: drill ≈ d − P, which gives about 77% thread (M6 → 5 mm, M8 → 6.8 mm, M10 → 8.5 mm)
How much thread do you need?
A full thread is rarely worth it: above about 75% the thread is barely stronger, but the tap needs much more torque and breaks more easily, especially in stainless steel, titanium and other tough materials. Most charts land near 75%: the usual metric drills (about d − P) give 74–82% and the standard inch chart sizes 65–81%. Lower percentages (60–65%) are common in hard or tough materials and for long engagements; higher ones mainly in thin sheet and soft materials. For metric threads, the hole must also stay within the 6H minor-diameter tolerance of ISO 965-1, which the results check.
Pipe threads
- G (BSPP, ISO 228-1): parallel threads that seal with a washer or O-ring on the face; 55° Whitworth form
- R / Rc / Rp (BSPT, ISO 7-1): taper 1 : 16 threads that seal on the thread with sealant; same form and pitch as G
- NPT (ASME B1.20.1): American 60° taper threads, also 1 : 16, sealed with tape or compound
- Taper threads are drilled and then tapped to depth with a gauge; a taper pipe reamer makes the larger sizes easier. The pitch, number of threads per inch and diameters are not the same between BSP and NPT — 1/2″ is 14 TPI in both, but the threads do not seal together
Clearance holes
ISO 273 gives three clearance-hole series for metric bolts: fine (close location), medium (the usual choice) and coarse (for loose fits or misaligned holes). For an M10 bolt they are 10.5, 11 and 12 mm. The tool shows them for metric sizes from M1.6 to M64.
Sources
- ISO 68-1:1998 and ISO 724:1993 — ISO metric thread basic profile and dimensions; ISO 261 and ISO 262 — selected sizes
- ISO 965-1 — tolerances (6H minor diameter)
- ISO 2306:1972, Drills for use prior to tapping screw threads
- ASME B1.1-2019, Unified Inch Screw Threads; ASME B1.20.1, Pipe Threads, General Purpose, Inch
- ISO 228-1 and ISO 7-1 — pipe threads where pressure-tight joints are not / are made on the threads
- ISO 273:1979, Fasteners — Clearance holes for bolts and screws
- Machinery’s Handbook, 32nd ed. — percentage of thread
Limitations
- Drills usually cut slightly oversize, more so in soft materials, which lowers the real thread percentage a little. Check a test hole for critical work.
- The usual drills come from common charts; tap makers sometimes recommend slightly different sizes for a particular tap and material — follow theirs when you have it.
- Tolerance checks cover the metric 6H class only. Inch class 2B/3B limits, tolerance classes 4H–7H and thread engagement length are not covered.
- Pipe-thread drills are the common shop sizes; taper threads also depend on how deep you tap.
Privacy
Everything happens in your browser. What you enter or open here is not uploaded or stored by MySmartCoPilot.
Frequently asked questions
What size drill do I need for an M6, M8 or M10 tap?
For standard (coarse) threads: M3 2.5 mm, M4 3.3 mm, M5 4.2 mm, M6 5.0 mm, M8 6.8 mm, M10 8.5 mm, M12 10.2 mm, M16 14 mm, M20 17.5 mm. They follow the rule drill ≈ diameter − pitch.
What does 75% thread mean?
How deep the thread is compared with a full-depth thread. A smaller drill gives a higher percentage and a stronger but harder-to-tap thread. Machinery’s Handbook gives % = 76.98 × (d − drill) ÷ P.
What drill size is used for a 1/4″-20 tap?
A #7 drill (0.201″, 5.1 mm), which gives about 75% thread. For 1/4″-28 UNF use a #3 drill (0.213″).
Do forming (roll) taps need a different drill?
Yes, a larger one, because the tap displaces the material instead of cutting it: about d − 0.0068 × P × %. For M6 at 65% that is 5.56 mm, against 5.0 mm for a cutting tap.
Is BSP the same as NPT?
No. BSP uses a 55° thread form and NPT a 60° form, and most sizes have different pitches. Even 1/2″, which is 14 TPI in both, will not seal reliably if you mix them.
What clearance hole should I use for an M8 bolt?
ISO 273 gives 8.4 mm (fine), 9 mm (medium) and 10 mm (coarse). Medium is the usual choice for general work.