Skip to content

M5 × 0.8

M5 thread pitch 0.8 mm and 4.2 mm tap drill size

ISO metric coarse thread · Ø 5 mm, pitch 0.8 mm · ISO 261 · ISO 68-1 · ISO 965

M5 × 0.8 is the standard metric thread for 5 mm: if a drawing just says "M5", 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
5 mm
Pitch PCoarse pitch, single start: advances one pitch per turn
0.8 mm
Profile angle
60°
Tensile stress area AsUsed to calculate the bolt load
14.2 mm²

Basic diameters

Pitch Ø d₂ = D₂
4.48 mm
Screw minor Ø d₃
4.019 mm
Nut minor Ø D₁
4.134 mm
Fundamental triangle height H
0.693 mm

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

d = 5d₂ = 4.48d₃ ≈ 4.019P = 0.860°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 H0.693 mm
ScaleNTS · mm

Where it is used

M5 pneumatic fittings, aluminium extrusion with T-nuts, brackets, covers and fixtures. An M5 socket head cap screw takes a 4 mm hex key and an M5 nut an 8 mm wrench. On machines of American origin, a “5 mm” hole may really be #10-24 or #10-32: measure the pitch before tapping or fitting a screw.

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 M5 × 0.8.

PartDiameterMinimumMaximum
Screw 6gMajor Ø d4.8264.976
Screw 6gPitch Ø d₂4.3614.456
Hole 6HPitch Ø D₂4.4804.605
Hole 6HMinor Ø D₁4.1344.334

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
4.2 mm
Form-tap drillGuide value: confirm with the tap maker
4.6 mm
Threading feedG95 F0.8 · in G94, F = RPM × pitch
0.8 mm/rev

Useful thread depth (guide)

Steel1–1.5 × d5–7.5 mm
Cast iron1.5 × d7.5 mm
Aluminium and soft metals2 × d10 mm

In a blind hole, drill deeper: useful thread + about 3 pitches for the tap lead and chips + the drill point. Steel example: 7.5 + 2.4 + 1.3 ≈ 12 mm.

4.2 mm drill. The cutting-tap drill is 4.2 mm. In soft aluminium, tapping with the correct drill and a sharp tap gives a better thread than opening up the hole. In blind holes, calculate the drilled depth separately from the useful thread: the tap’s chamfer does not cut a full thread in its first turns.

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
3.25°
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 →

M5 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
5.3 mm
MediumMost common
5.5 mm
Coarse
5.8 mm

Head recess

Counterbore for socket head cap screw (ISO 4762)DIN 974-1
Ø10 × 5.4
90° countersink (DIN 7991)
Ø10.4

Wrench sizes

Hex head and nut (ISO 4017 / 4032)
8 mm
Socket head cap screw (ISO 4762)
4 mm
Countersunk socket screw (DIN 7991)
3 mm

Tightening torque (guide)

Grade 8.8
5.5 N·m
Grade 10.9
8.1 N·m
Grade 12.9
9.5 N·m

Steel screw tightened to 90 % of yield with friction μ = 0.12 (no special lubrication). Oil, zinc plating or aluminium change it: the maker's table rules.

If the thread strips

Helical insert (HeliCoil / Recoil)
M5 × 0.8 STI
STI tap drillAs supplied in insert kits
5.2 mm
Usual insert length2 × d or more in aluminium
1.5 × d = 7.5 mm

With the insert the thread is M5 × 0.8 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 M5 × 0.8

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 M5 reads between 4.826 and 4.976 mm (a little less if worn).
  2. 2. Check the pitchA 0.8 mm pitch gauge should show no light between the teeth. Without a gauge: 12.5 threads in 10 mm.
  3. 3. If it's a tapped holeThe minor diameter is about 4.134–4.334 mm. Quickest check: try a known-good M5 screw.

Threads confused with M5 × 0.8

ThreadØ mmPitch mmTPIHow to tell
M5 × 0.850.831.8This page
#10-32 UNF4.8260.79432Nearly the same pitch (0.794 mm); Ø reads 4.83 mm
BSF 3/16"-324.7630.79432Nearly the same pitch (0.794 mm); Ø reads 4.76 mm; 55° profile
2 BA4.70.8131.4Nearly the same pitch (0.81 mm); Ø reads 4.7 mm; 47.5° profile
#12-32 UNEF5.4860.79432Nearly the same pitch (0.794 mm); Ø reads 5.49 mm
1 BA5.30.928.25.3 mm Ø and 0.9 mm pitch; 47.5° profile
Identify a thread from your measurements →

Frequently asked questions

What drill is used for M5?+

4.2 mm for a cutting tap. A form tap needs a larger hole (about 4.6 mm); confirm it with the tap’s data.

What is the pitch of M5?+

The coarse pitch is 0.8 mm. M5 × 0.5 fine pitch also exists.

Is M5 the same as #10-24 or #10-32?+

No. #10 threads are 4.826 mm with 24 or 32 threads per inch (1.058 or 0.794 mm pitch). They are not interchangeable with M5.

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; tightening torque, Technical information: screws and nuts (μ = 0.12). Reference data: the drawing, tolerance class and maker's instructions govern. A cutting-tap drill is not for form tapping. Reviewed on .