Tap drill size controls how much material remains for the tap to cut or form. A smaller hole generally increases thread engagement and tapping torque; a larger hole reduces engagement. The useful starting formula depends on whether the tap cuts material or displaces it.
Common metric shop rule: tap drill ≈ major diameter − pitch.
Metric percentage estimate: drill = D − (% thread × pitch ÷ 76.98).
Unified percentage estimate: drill = D − (0.01299 × % thread ÷ TPI).
The diameter-minus-pitch shop rule
For a standard 60-degree metric cut thread, subtracting pitch from nominal diameter gives a convenient starting drill. For M10 × 1.5:
The rule is useful because metric pitch is already expressed as axial distance between adjacent thread crests. It is still an approximation: actual engagement depends on the finished hole, tap geometry, tolerance class, and process variation.
Percentage-of-thread formulas
When a different engagement target is needed, Guhring publishes geometry-based formulas for 60-degree cut taps:
These equations estimate geometric engagement. The actual percentage can differ because the drilled hole may run oversize, the tap may cut oversize, and thread class and material behavior affect the finished thread.
Worked tap drill examples
M10 × 1.5 at 75% estimated engagement
Drill = 10 − (75 × 1.5 ÷ 76.98) = 8.5386 mm. A commonly stocked 8.5 mm drill is close to the estimate. The final choice should follow the tap manufacturer and tolerance requirement.
1/4-20 UNC at 75% estimated engagement
Drill = 0.250 − (0.01299 × 75 ÷ 20) = 0.2013 in. A number 7 drill is 0.2010 in and is a common cut-tap starting size.
| Thread | Formula estimate | Common nearby drill |
|---|---|---|
| M10 × 1.5 | 8.5386 mm | 8.5 mm |
| 1/4-20 UNC | 0.2013 in | #7 / 0.2010 in |
Use the Metric, UNC & UNF Tap Drill Chart for common stocked designations and decimal equivalents.
Cut taps and form taps need different holes
A cut tap removes material to generate the internal thread. A form or roll tap displaces material, so it generally needs a larger pre-tap hole and a manufacturer-specific recommendation. Applying a cut-tap formula to a form tap can produce excessive torque, poor thread formation, tap failure, or an out-of-tolerance thread.
Do not assume one form-tap formula covers every material. Ductility, hole finish, lubrication, coating, thread class, and tap design are especially important.
How to select the production drill
- Identify cut tap versus form tap.
- Confirm nominal diameter, pitch or TPI, thread series, and required class.
- Start with the tap manufacturer’s published hole range.
- Account for material, coating, lubrication, hole depth, blind-hole clearance, and chip evacuation.
- Measure the actual drilled hole rather than relying only on drill marking.
- Verify the finished thread with the specified gage and inspection plan.
Why more engagement is not always better
Increasing engagement leaves more material for the tap to remove and usually increases torque. Beyond the required functional thread, extra engagement can reduce reliability without producing a proportional strength benefit. The correct target belongs to the drawing, applicable standard, engineering requirement, and tap manufacturer—not to a universal “maximum thread” rule.
Technical references
Published and formula-checked by MfgWorkbench. Last reviewed September 4, 2026. See our editorial method.