How to use this calculator
- Choose the thread. Select the thread size; its major diameter and pitch are set automatically.
- Set the % thread engagement. Enter the target percentage — 60–75% is typical.
- Read the tap drill. Read the tap drill diameter and use the nearest available drill at or just above it.
How it works
The tap drill leaves enough material for the tap to cut threads to a chosen depth — the percent of thread engagement. The drill diameter is: tap drill = major − (%thread × pitch) / 76.98 The constant 76.98 comes from the 60° thread geometry, and it is the convention printed on tap-drill charts. The familiar shortcut “tap drill = major − pitch” is just this formula at about 77% thread.
The nearest-drill result rounds metric threads to a common 0.1 mm drill and unified threads to the closest number, letter or fractional shop drill. Treat it as a starting recommendation: in hard materials, blind holes or small taps, choose the slightly larger practical drill when tapping torque is the limiting risk. For a static table view, use the tap drill chart; for thread geometry beyond the drill hole, use the thread pitch diameter calculator. The hole this drill makes must land inside the class 2B minor-diameter band — the unified thread limits calculator computes that band (and every other 2A/2B limit) for any diameter-TPI from the B1.1 formulas.
Higher engagement is not better: most of a thread’s strength is in the first few threads, so going from 65% to 75% roughly doubles the tapping torque for a negligible strength gain. For hard materials, deep holes or small taps, 50–65% engagement taps far more safely.
After picking the drill, the next shop checks are feed and depth. Use the tapping feed rate calculator to set synchronized spindle feed, the drill point length calculator for blind-hole depth allowance, and the thread engagement calculator when the question is pull-out strength rather than tap torque.
Worked example
Verified against the live calculator
An M6 thread has a 1 mm pitch. At 75% engagement the tap drill is
6 − (75 × 1) / 76.98 ≈ 5.03 mm, so you would use a 5.0 mm drill — the
classic M6 tap drill. The basic minor diameter is 6 − 1.0825 × 1 ≈ 4.92 mm.
The calculator returns these directly and shows 5.0 mm as the
nearest common metric drill.
Reference data
Standard threads with their major diameter, pitch and the tap drill at 75% engagement.
| Thread | Major Ø (mm) | Pitch (mm) | Tap drill @75% (mm) | Nearest drill |
|---|---|---|---|---|
| M3 | 3 | 0.5 | 2.51 | 2.5 mm |
| M4 | 4 | 0.7 | 3.32 | 3.3 mm |
| M5 | 5 | 0.8 | 4.22 | 4.2 mm |
| M6 | 6 | 1 | 5.03 | 5.0 mm |
| M8 | 8 | 1.25 | 6.78 | 6.8 mm |
| M10 | 10 | 1.5 | 8.54 | 8.5 mm |
| M12 | 12 | 1.75 | 10.3 | 10.3 mm |
| M16 | 16 | 2 | 14.1 | 14.1 mm |
| M20 | 20 | 2.5 | 17.6 | 17.6 mm |
| M24 | 24 | 3 | 21.1 | 21.1 mm |
| M8x1 | 8 | 1 | 7.03 | 7.0 mm |
| M10x1.25 | 10 | 1.25 | 8.78 | 8.8 mm |
| M12x1.25 | 12 | 1.25 | 10.8 | 10.8 mm |
| #10-24 UNC | 4.826 | 1.0583 | 3.79 | #25 |
| 1/4-20 UNC | 6.35 | 1.27 | 5.11 | #7 |
| 5/16-18 UNC | 7.9375 | 1.4111 | 6.56 | F |
| 3/8-16 UNC | 9.525 | 1.5875 | 7.98 | 5/16" |
| 1/2-13 UNC | 12.7 | 1.9538 | 10.8 | 27/64" |
| 1/4-28 UNF | 6.35 | 0.9071 | 5.47 | #3 |
| 3/8-24 UNF | 9.525 | 1.0583 | 8.49 | Q |
Source: ISO 261/262 (metric) and ASME B1.1 (unified). Verify against a current tap-drill chart and your tap maker's recommendation.
Frequently asked questions
How do I calculate tap drill size?
Tap drill = major diameter − (%thread × pitch) ÷ 76.98 for 60° threads. For an M6 (1 mm pitch) at 75% thread that is 6 − 0.97 ≈ 5.0 mm. The calculator also suggests the nearest common metric or inch-series shop drill.
What percentage of thread engagement should I use?
About 75% is the traditional default, but 60–65% is plenty for most jobs and taps far more easily, with very little loss of strength. Drop toward 50% in hard materials or deep holes.
Is 75% thread really necessary?
Rarely. Almost all of a thread’s strength is carried by the first few engaged threads, and going from 65% to 75% roughly doubles the tapping torque for only a few percent more strength. Higher % mainly raises tap-breakage risk.
What is the tap drill for M6, M8 and M10?
At about 75% thread: M6 → 5.0 mm, M8 → 6.8 mm, M10 → 8.5 mm. See the table for the full list and pick the nearest available drill.
What is the minor diameter?
The basic internal minor diameter is major − 1.0825 × pitch — the diameter at 100% thread form. Tap drills sit above it because real threads do not need to be cut to a perfect sharp root.
Does this cover metric and inch threads?
Yes — metric coarse and fine plus unified UNC/UNF. Toggle SI/Imperial to read the drill size in mm or inches.
Method & assumptions
- 60° ISO/Unified threads; the % thread uses the chart convention (76.98 constant).
- Cut taps — roll/form taps need a larger hole (no chips removed); follow the form-tap maker’s chart.
- Round up to the nearest available drill; under-size holes raise torque and break taps.