Skip to content

M12 × 1.75

M12 thread pitch 1.75 mm and 10.2 mm tap drill size

ISO metric coarse thread · Ø 12 mm, pitch 1.75 mm · ISO 261 · ISO 68-1 · ISO 965

M12 × 1.75 is the standard metric thread for 12 mm: if a drawing just says "M12", 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
12 mm
Pitch PCoarse pitch, single start: advances one pitch per turn
1.75 mm
Profile angle
60°
Tensile stress area AsUsed to calculate the bolt load
84.3 mm²

Basic diameters

Pitch Ø d₂ = D₂
10.863 mm
Screw minor Ø d₃
9.853 mm
Nut minor Ø D₁
10.106 mm
Fundamental triangle height H
1.516 mm

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

d = 12d₂ = 10.863d₃ ≈ 9.853P = 1.7560°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 H1.516 mm
ScaleNTS · mm

Where it is used and its fine pitches

Machine bases, brackets, eye bolts, clamps and studs. There are three common pitches: 1.75 (coarse), 1.5 and 1.25 (fine, typical of automotive and hydraulics). An M12 socket head cap screw takes a 10 mm hex key and the nut an 18 mm wrench (19 mm in the old DIN 934).

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 M12 × 1.75.

PartDiameterMinimumMaximum
Screw 6gMajor Ø d11.70111.966
Screw 6gPitch Ø d₂10.67910.829
Hole 6HPitch Ø D₂10.86311.063
Hole 6HMinor Ø D₁10.10610.441

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
10.2 mm
Form-tap drillGuide value: confirm with the tap maker
11.1 mm
Threading feedG95 F1.75 · in G94, F = RPM × pitch
1.75 mm/rev

Useful thread depth (guide)

Steel1–1.5 × d12–18 mm
Cast iron1.5 × d18 mm
Aluminium and soft metals2 × d24 mm

In a blind hole, drill deeper: useful thread + about 3 pitches for the tap lead and chips + the drill point. Steel example: 18 + 5.3 + 3.1 ≈ 27 mm.

10.2 mm drill. For a cutting tap, 10.2 mm. In tough materials or in production, use rigid tapping and coolant; on large parts or hard materials, thread milling avoids the risk of breaking a tap inside an expensive part.

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
2.94°
Shim plateThe holder already has 1°; the shim adds +2°
3°
External thread codeInsert size 16
AE16+2
Internal thread code
AI16+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 →

M12 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
13 mm
MediumMost common
13.5 mm
Coarse
14.5 mm

Head recess

Counterbore for socket head cap screw (ISO 4762)DIN 974-1
Ø20 × 13
90° countersink (DIN 7991)
Ø24.4

Wrench sizes

Hex head and nut (ISO 4017 / 4032)With DIN 933 / 934: 19 mm
18 mm
Socket head cap screw (ISO 4762)
10 mm
Countersunk socket screw (DIN 7991)
8 mm

Tightening torque (guide)

Grade 8.8
80 N·m
Grade 10.9
117 N·m
Grade 12.9
137 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)
M12 × 1.75 STI
STI tap drillAs supplied in insert kits
12.5 mm
Usual insert length2 × d or more in aluminium
1.5 × d = 18 mm

With the insert the thread is M12 × 1.75 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 M12 × 1.75

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 M12 reads between 11.701 and 11.966 mm (a little less if worn).
  2. 2. Check the pitchA 1.75 mm pitch gauge should show no light between the teeth. Without a gauge: 5.7 threads in 10 mm.
  3. 3. If it's a tapped holeThe minor diameter is about 10.106–10.441 mm. Quickest check: try a known-good M12 screw.

Threads confused with M12 × 1.75

ThreadØ mmPitch mmTPIHow to tell
M12 × 1.75121.7514.5This page
BSW 7/16"-1411.1131.81414Nearly the same pitch (1.814 mm); Ø reads 11.11 mm; 55° profile
7/16"-14 UNC11.1131.81414Nearly the same pitch (1.814 mm); Ø reads 11.11 mm
M12 × 1.5121.516.9Same Ø, 1.5 mm pitch: the gauge won't seat
BSF 1/2"-1612.71.58816Nearly the same pitch (1.588 mm); Ø reads 12.7 mm; 55° profile
1/2"-13 UNC12.71.9541312.7 mm Ø and 1.954 mm pitch
Identify a thread from your measurements →

Frequently asked questions

What drill is used for M12?+

10.2 mm for a cutting tap. A form tap needs a larger hole (about 11.1 mm); confirm it with the tap’s data.

What is the pitch of M12?+

The coarse pitch is 1.75 mm. The common fine pitches are 1.5 and 1.25 mm.

Are M12 and 1/2-13 UNC interchangeable?+

No. 1/2-13 UNC is 12.7 mm with a 1.954 mm pitch. They look alike but do not thread into each other.

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 .