Skip to content

M16 × 2

M16 thread pitch 2 mm and 14 mm tap drill size

ISO metric coarse thread · Ø 16 mm, pitch 2 mm · ISO 261 · ISO 68-1 · ISO 965

M16 × 2 is the standard metric thread for 16 mm: if a drawing just says "M16", 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
16 mm
Pitch PCoarse pitch, single start: advances one pitch per turn
2 mm
Profile angle
60°
Tensile stress area AsUsed to calculate the bolt load
156.7 mm²

Basic diameters

Pitch Ø d₂ = D₂
14.701 mm
Screw minor Ø d₃
13.546 mm
Nut minor Ø D₁
13.835 mm
Fundamental triangle height H
1.732 mm

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

d = 16d₂ = 14.701d₃ ≈ 13.546P = 260°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 H1.732 mm
ScaleNTS · mm

Where it is used

Frames, anchors, lifting eye bolts, flanges and machine bases. An M16 socket head cap screw takes a 14 mm hex key and the nut a 24 mm wrench. The usual fine pitch is M16 × 1.5, common in hydraulics and lock nuts.

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 M16 × 2.

PartDiameterMinimumMaximum
Screw 6gMajor Ø d15.68215.962
Screw 6gPitch Ø d₂14.50314.663
Hole 6HPitch Ø D₂14.70114.913
Hole 6HMinor Ø D₁13.83514.210

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
14 mm
Form-tap drillGuide value: confirm with the tap maker
15 mm
Threading feedG95 F2 · in G94, F = RPM × pitch
2 mm/rev

Useful thread depth (guide)

Steel1–1.5 × d16–24 mm
Cast iron1.5 × d24 mm
Aluminium and soft metals2 × d32 mm

In a blind hole, drill deeper: useful thread + about 3 pitches for the tap lead and chips + the drill point. Steel example: 24 + 6 + 4.2 ≈ 35 mm.

14 mm drill and tapping torque. For a cutting tap, 14 mm. An M16 tap takes a lot of torque: on a machining centre use rigid tapping with plenty of coolant and check that the spindle and taper can take it. On expensive parts or hard materials, thread milling is safer and lets you adjust size with the offset.

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
2.48°
Shim plateThe holder already has 1°; the shim adds +1°
2°
External thread codeInsert size 16
AE16+1
Internal thread code
AI16+1

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 →

M16 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
17 mm
MediumMost common
17.5 mm
Coarse
18.5 mm

Head recess

Counterbore for socket head cap screw (ISO 4762)DIN 974-1
Ø26 × 17.5
90° countersink (DIN 7991)
Ø32.4

Wrench sizes

Hex head and nut (ISO 4017 / 4032)
24 mm
Socket head cap screw (ISO 4762)
14 mm
Countersunk socket screw (DIN 7991)
10 mm

Tightening torque (guide)

Grade 8.8
194 N·m
Grade 10.9
285 N·m
Grade 12.9
333 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)
M16 × 2 STI
STI tap drillAs supplied in insert kits
16.5 mm
Usual insert length2 × d or more in aluminium
1.5 × d = 24 mm

With the insert the thread is M16 × 2 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 M16 × 2

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 M16 reads between 15.682 and 15.962 mm (a little less if worn).
  2. 2. Check the pitchA 2 mm pitch gauge should show no light between the teeth. Without a gauge: 5 threads in 10 mm.
  3. 3. If it's a tapped holeThe minor diameter is about 13.835–14.21 mm. Quickest check: try a known-good M16 screw.

Threads confused with M16 × 2

ThreadØ mmPitch mmTPIHow to tell
M16 × 216212.7This page
BSF 5/8"-1415.8751.81414Nearly the same pitch (1.814 mm); Ø reads 15.88 mm; 55° profile
BSW 5/8"-1115.8752.3091115.88 mm Ø and 2.309 mm pitch; 55° profile
5/8"-11 UNC15.8752.3091115.88 mm Ø and 2.309 mm pitch
M16 × 1.5161.516.9Same Ø, 1.5 mm pitch: the gauge won't seat
5/8"-18 UNF15.8751.4111815.88 mm Ø and 1.411 mm pitch
Identify a thread from your measurements →

Frequently asked questions

What drill is used for M16?+

14 mm for a cutting tap. A form tap needs a larger hole (about 15 mm); confirm it with the tap maker.

What is the pitch of M16?+

The coarse pitch is 2 mm. The most used fine pitch is 1.5 mm.

Is it better to tap or thread mill M16?+

In production and ordinary steel, tapping is faster. On expensive parts, hard materials or when size must be adjusted, thread milling is safer.

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 .