Home / Guides / Design

Specifying threads so they come back the way you expect

August 14, 2026

Threads look like the simplest feature on a drawing and they generate more quoting questions than anything except tolerances. The reason is that a thread callout carries at least five decisions and most drawings only state two of them.

What a complete callout contains

A thread line a shop can machine without asking looks like this:

M6 x 1.0 - 6H, full thread depth 12 mm, drill depth 16 mm, 4 places, per ISO 965

It states the size, the pitch, the tolerance class, the depth of full thread, the depth of the drilled hole, the quantity and the standard. Compare that with “M6 tapped hole”, which leaves the shop to guess the depth, the class and whether the hole is blind or through.

For imperial work the same applies: name the series and the class, for example 1/4-20 UNC-2B, and say whether it is a through hole.

Engagement depth, not hole depth

Engagement is where strength comes from, and it stops growing usefully after a point.

Material	Practical engagement
Steel and stainless	1.0 x diameter
Cast iron and brass	1.25 x diameter
Aluminium	1.5 x diameter
POM, nylon, PEEK	2.0 x diameter

A blind hole needs extra depth below the full thread for the tap to run out, typically two to three pitches for a standard tap. If your drawing calls for full thread all the way to the bottom of a blind hole, the shop has to use a bottoming tap, run slowly and accept a higher risk of a broken tap in the part, which usually means scrapping it.

Tapping and thread milling

Tapping drives a tap into the hole. Fast, cheap and standard for small sizes in soft materials. The risks are broken taps in blind holes and poor chip evacuation in gummy materials such as stainless and some aluminium alloys.

Thread milling uses a rotating cutter to spiral the thread. It works in hard materials, produces a better finish, can cut several diameters with one tool and leaves a recoverable situation if something goes wrong. It is slower per hole on small sizes.

Most shops decide by size and material without being told. Where you should care is on large threads, on hardened parts and on high value parts where a broken tap means scrapping an expensive component. On those, writing “thread milling preferred” is reasonable.

Threaded inserts

Threads in aluminium and plastic wear. If a cover comes off during service several times a year, the thread will eventually fail and the housing is scrap.

Two common answers:

• Helical wire inserts are cheap, installed with a simple tool, and turn an M4 thread in aluminium into something close to steel strength. They need a specific oversized tapped hole, so the drawing must call out the insert part number and the corresponding tap.
• Press-in and heat-set inserts are used in plastics, particularly for assemblies that come apart. Heat-set inserts need a boss with the right internal diameter and wall thickness, which the insert manufacturer specifies.

Whichever you choose, put the insert specification on the drawing and say whether the shop supplies and installs them or whether you do. This is one of the most common gaps between a quote and an invoice.

Practical details that avoid rejects

• Chamfer the thread entry. A small chamfer helps the tap start straight and stops the first thread lifting a burr. Call it out.
• Say whether threads are masked during finishing. Anodising builds inside a thread and can make it unusable for a fastener. Either mask or chase after finishing, and state which.
• Do not tolerance thread positions tighter than they need. A clearance hole in the mating part is cheaper than a positional tolerance on eight tapped holes.
• Consolidate sizes. One thread size across a part means one tap, one tool change and one gauge in inspection.
• Say how they will be checked. Go and no-go gauges are the norm. If you expect a gauge report, say so up front.

Quick reference for common sizes

Depths below are working figures for a blind hole in aluminium, which is the most common case in the requests we see.

Thread	Tap drill	Full thread depth	Minimum drill depth
M3 x 0.5	2.5 mm	4.5 mm	7 mm
M4 x 0.7	3.3 mm	6 mm	9 mm
M5 x 0.8	4.2 mm	7.5 mm	11 mm
M6 x 1.0	5.0 mm	9 mm	13 mm
M8 x 1.25	6.8 mm	12 mm	17 mm

Steel needs less engagement, plastics need more. Treat the table as a starting point and state the depth you want on the drawing rather than leaving it to be inferred.

What to do when a tap breaks

It happens, particularly in stainless and in deep blind holes. What matters is what the shop does next.

A serious shop tells you, and offers one of three routes: remove the tap with EDM and re-tap, scrap the piece and remake it, or, if the thread is non critical, propose a documented deviation. A shop that quietly fills the hole and ships it is one you find out about later, in an assembly line, with no explanation available.

Asking “what is your procedure when a tap breaks in a nearly finished part” during vetting gets a surprisingly informative answer. It is a question only someone who has bought machined parts before would ask.

Threads rarely break a quote on their own, but they are a good test of a shop. A shop that comes back asking about engagement depth and blind hole runout is reading your drawing properly. That is the kind of question the guide on vetting a machine shop says to look for, and you can send your drawing here when you want it read by shops in Vietnam.

Questions we get on this

Keep reading

• What a DFM review actually changes, with the numbers
• Twelve design changes that take real money out of a machined part