Skip to content
Steel Wing
← Technical Notes
Threading

Tap drill size chart: metric, fine, UNC/UNF and G threads — the right drill diameter before tapping

Tap drill diameters for M1.6–M30, UNC/UNF and G (BSP) threads; how percent thread affects torque and strength; why forming taps need a larger hole.

November 10, 20264 min readSteel Wing

The most common cause of tap breakage is not the tap but the hole. A hole drilled 0.2 mm undersize noticeably raises the volume of material the tap must remove and the torque it must carry; even an HSS-E tap will break. This note collects the chart every shop looks up daily and explains the logic behind it.

Rule of thumb: drill diameter ≈ thread diameter − pitch

For metric threads the practical rule for the tap drill is:

D1 ≈ D − P (D: nominal thread diameter, P: pitch)

For M8 × 1.25: 8 − 1.25 = 6.75 → Ø 6.8 mm drill. For M10 × 1.5: 10 − 1.5 = 8.5 mm. With a standard 6H tolerance this gives about 75 % thread height and matches the DIN 336 tables.

Thread profile: D nominal diameter, P pitch, D1 minor (drill) diameter. Drill ≈ D − P.
Thread profile: D nominal diameter, P pitch, D1 minor (drill) diameter. Drill ≈ D − P.

Metric coarse (M) — DIN 13

ThreadPitch (mm)Drill Ø (mm)
M1.60.351.25
M20.401.60
M2.50.452.05
M30.502.50
M40.703.30
M50.804.20
M61.005.00
M81.256.80
M101.508.50
M121.7510.20
M142.0012.00
M162.0014.00
M182.5015.50
M202.5017.50
M222.5019.50
M243.0021.00
M273.0024.00
M303.5026.50

Metric fine (MF)

ThreadDrill Ø (mm)
M8 × 17.00
M10 × 1.258.80
M10 × 19.00
M12 × 1.510.50
M12 × 1.2510.80
M14 × 1.512.50
M16 × 1.514.50
M18 × 1.516.50
M20 × 1.518.50
M24 × 222.00
M30 × 228.00

UNC / UNF (inch)

ThreadDrill (inch)Drill Ø (mm)
1/4-20 UNC#75.10
5/16-18 UNCF6.50
3/8-16 UNC5/167.90
7/16-14 UNCU9.35
1/2-13 UNC27/6410.70
5/8-11 UNC17/3213.50
3/4-10 UNC21/3216.70
1/4-28 UNF#35.40
5/16-24 UNFI6.90
3/8-24 UNFQ8.40
1/2-20 UNF29/6411.50
5/8-18 UNF37/6414.70

G (BSP) pipe thread — parallel

ThreadTPIDrill Ø (mm)
G 1/8288.80
G 1/41911.80
G 3/81915.30
G 1/21419.00
G 3/41424.50
G 11130.75

The G values are DIN 336 recommended drills; some charts give the minor diameter instead (e.g. 18.6 mm for G 1/2) and both conventions are in use. For tapered pipe threads such as NPT and NPTF the hole depends on thread depth and taper; use the tap manufacturer's own chart. Critical sealing threads must be gauged.

Percent thread: aim for 60–75 %, not 100 %

Many operators drill small because "a full thread is stronger". The opposite is true:

  • Going from 75 % to 100 % thread height raises the tensile strength of the thread by only about 5 %.
  • The same change raises tapping torque 2–3 times. That is where breakage, wear and torn threads come from.
  • Steel and stainless: 65–75 %. Aluminium and ductile materials: 60–70 %. Cast iron may go to 75–80 %.
Thread height 100 % / 75 % / 60 %: torque and breakage risk drop fast while thread strength stays almost constant.
Thread height 100 % / 75 % / 60 %: torque and breakage risk drop fast while thread strength stays almost constant.

The chart values target exactly this band. A smaller hole does the tap no favour.

Forming (fluteless) taps: drill the hole larger

A forming tap removes no chips; it flows the material plastically into the thread profile. Because the crest is built from displaced material, the hole is drilled larger than for a cutting tap:

ThreadCutting tap ØForming tap Ø
M32.502.80
M43.303.70
M54.204.60
M65.005.50
M86.807.40
M108.509.30
M1210.2011.10

Using a forming tap in a hole drilled to the cutting chart almost guarantees breakage. Forming taps are only for ductile materials (aluminium, copper alloys, low-carbon steel, austenitic stainless) with elongation above about 8 %; never in cast iron. Forming-tap drill sizes vary by about ±0.1 mm between manufacturers and target thread height; the tap maker's chart governs.

M8 hole difference: cutting tap (Ø 6.8) versus forming tap (Ø 7.4).
M8 hole difference: cutting tap (Ø 6.8) versus forming tap (Ø 7.4).

Three cases outside the chart

  1. Plated threads: if a bolt must fit after zinc or phosphate plating, use a 6G-tolerance tap and one drill size up.
  2. Blind-hole depth: hole depth = thread depth + tap chamfer length + chip room. With a spiral-flute tap leave at least 2–3 pitches of clearance.
  3. Drill wear: a worn drill cuts undersize. If tap breakage increases, measure the drill diameter with a micrometer first.

Quick checklist

  • Drill size taken from the chart and checked with D − P.
  • Cutting or forming? Forming uses the larger chart.
  • Depth allowance left in blind holes.
  • 6G chosen where the thread is plated afterwards.
  • Critical threads verified with a go / no-go gauge.

Chart values are reference values consistent with DIN 336 and common manufacturer catalogues; for special tolerances use the manufacturer's table. Steel Wing supplies MCI Tool machine taps from stock in HSS-E and HSS-E-PM, spiral-flute, spiral-point and forming types; let us select the right size and type for your application together.

Looking for a quote on your project?

Tell us about your manufacturing or cutting-tool needs and our engineering team will get back to you promptly.

Get in Touch