Skip to content

M3 × 0.5

M3 thread pitch 0.5 mm and 2.5 mm tap drill size

ISO metric coarse thread · Ø 3 mm, pitch 0.5 mm · ISO 261 · ISO 68-1 · ISO 965

M3 × 0.5 is the standard metric thread for 3 mm: if a drawing just says "M3", this is it. Here are its dimensions, tolerances, how to drill and tap it, the matching fasteners and how to repair it.

Thread dimensions

Designation

Nominal diameter d
3 mm
Pitch PCoarse pitch, single start: advances one pitch per turn
0.5 mm
Profile angle
60°
Tensile stress area AsUsed to calculate the bolt load
5 mm²

Basic diameters

Pitch Ø d₂ = D₂
2.675 mm
Screw minor Ø d₃
2.387 mm
Nut minor Ø D₁
2.459 mm
Fundamental triangle height H
0.433 mm

Basic values without tolerance: the actual manufacturing limits are in the next section.

d = 3d₂ = 2.675d₃ ≈ 2.387P = 0.560°Haxis
d
Major Ø. Crest to crest; what calipers read.
d₂
Pitch Ø. Sets the fit; what gauges check.
d₃
Root Ø. Thinnest part of the screw.
P
Pitch. Advance per turn.
H
Theoretical height. Of the sharp-V profile.
PartBasic profile
StandardISO 68-1
Height H0.433 mm
ScaleNTS · mm

Where it is used

Small electronics hardware, sheet-metal covers, sensors, light fixtures and circuit boards. An M3 socket head cap screw (ISO 4762) takes a 2.5 mm hex key and a standard M3 nut a 5.5 mm wrench: useful hints, but no substitute for measuring the pitch.

Tolerances 6H / 6g

If the drawing gives no class, the medium class applies: 6H for the nut or tapped hole and 6g for the screw. These are the limits for M3 × 0.5.

PartDiameterMinimumMaximum
Screw 6gMajor Ø d2.8742.980
Screw 6gPitch Ø d₂2.5802.655
Hole 6HPitch Ø D₂2.6752.775
Hole 6HMinor Ø D₁2.4592.599

The pitch diameter is checked with go / no-go gauges or the three-wire method; calipers only give the major diameter. Limits per ISO 965-2.

Drill and tap

Drills and feed

Cutting-tap drillVÖLKEL · Metric cutting taps
2.5 mm
Form-tap drillGuide value: confirm with the tap maker
2.75 mm
Threading feedG95 F0.5 · in G94, F = RPM × pitch
0.5 mm/rev

Useful thread depth (guide)

Steel1–1.5 × d3–4.5 mm
Cast iron1.5 × d4.5 mm
Aluminium and soft metals2 × d6 mm

In a blind hole, drill deeper: useful thread + about 3 pitches for the tap lead and chips + the drill point. Steel example: 4.5 + 1.5 + 0.8 ≈ 7 mm.

2.5 mm drill and how not to break the tap. With a cutting tap, drill 2.5 mm. In blind holes leave extra depth below the useful thread and use a spiral-flute tap to lift the chips; in through holes, a spiral-point tap. Lubricate well and, on a machine, use rigid tapping or a holder with a clutch: an M3 tap snaps before you feel the load.

Lathe threading: shim plate

Only if you single-point the thread on a lathe. The shim tilts the insert to follow the helix so it doesn't rub on one flank.

Helix angleCalculated on the pitch diameter
3.4°
Shim plateThe holder already has 1°; the shim adds +2°
3°
External thread codeInsert size 11
AE11+2
Internal thread code
AI11+2

For a right-hand thread with a right-hand holder. With a left-hand thread or the holder the other way round, the shim changes sign. Codes follow the usual threading-holder naming (AE external, AI internal): check your brand's catalogue.

Calculate the shim for your holder →

M3 fasteners and assembly

What you need for the part that takes the screw: clearance hole, head recess, wrench sizes and tightening torque.

Clearance hole (ISO 273)

Fine
3.2 mm
MediumMost common
3.4 mm
Coarse
3.6 mm

Head recess

Counterbore for socket head cap screw (ISO 4762)DIN 974-1
Ø6.5 × 3.3
90° countersink (DIN 7991)
Ø6.3

Wrench sizes

Hex head and nut (ISO 4017 / 4032)
5.5 mm
Socket head cap screw (ISO 4762)
2.5 mm
Countersunk socket screw (DIN 7991)
2 mm

If the thread strips

Helical insert (HeliCoil / Recoil)
M3 × 0.5 STI
STI tap drillAs supplied in insert kits
3.2 mm
Usual insert length2 × d or more in aluminium
1.5 × d = 4.5 mm

With the insert the thread is M3 × 0.5 again: the original screw still fits. If the joint is taken apart often or carries high torque, a solid insert lasts longer; if changing the screw is fine, you can also go up one size.

Calculate the insert repair →

How to tell it is M3 × 0.5

If you have the part or screw and don't know the thread, check the diameter first and then the pitch.

  1. 1. Measure the screw ODWith calipers on the crests. An M3 reads between 2.874 and 2.98 mm (a little less if worn).
  2. 2. Check the pitchA 0.5 mm pitch gauge should show no light between the teeth. Without a gauge: 20 threads in 10 mm.
  3. 3. If it's a tapped holeThe minor diameter is about 2.459–2.599 mm. Quickest check: try a known-good M3 screw.

Threads confused with M3 × 0.5

ThreadØ mmPitch mmTPIHow to tell
M3 × 0.530.550.8This page
#4-48 UNF2.8450.52948Nearly the same pitch (0.529 mm); Ø reads 2.85 mm
6 BA2.80.5347.9Nearly the same pitch (0.53 mm); Ø reads 2.8 mm; 47.5° profile
7 BA2.50.4852.9Nearly the same pitch (0.48 mm); Ø reads 2.5 mm; 47.5° profile
#5-44 UNF3.1750.577443.18 mm Ø and 0.577 mm pitch
#3-48 UNC2.5150.52948Nearly the same pitch (0.529 mm); Ø reads 2.52 mm
Identify a thread from your measurements →

Frequently asked questions

What drill is used for M3?+

2.5 mm for a cutting tap. A form tap needs a larger hole (about 2.75 mm): confirm it with the tap’s data.

What is the pitch of an M3 thread?+

The coarse pitch of M3 is 0.5 mm. There is also M3 × 0.35 fine pitch, which is much less common.

Are M3 and #4-40 UNC interchangeable?+

No. #4-40 is 2.845 mm with a 0.635 mm pitch: the screw may start a few turns, but it binds and damages the thread.

Sources: profile and diameters, ISO 68-1 and ISO 261; tolerances, ISO 965-2; drill, VÖLKEL · Metric cutting taps; clearance hole, ISO 273; counterbore, DIN 974-1; wrench sizes, ISO 4017, ISO 4032, ISO 4762 and DIN 7991. Reference data: the drawing, tolerance class and maker's instructions govern. A cutting-tap drill is not for form tapping. Reviewed on .