Types of Thread Taps and When Each One Is Used

Two ways to classify a tap

A tap is a hardened tool that cuts or forms a thread inside a hole. Beyond the thread size and pitch it is made for, taps differ in two independent ways, and both have to be right for the job.

The lead — the chamfered section at the tip — determines how close to the bottom of a blind hole the tap can cut a usable thread.

The flute geometry determines which direction the chips travel, and therefore whether the tap suits a through hole or a blind hole.

A tap is specified by both. A plug-lead spiral flute tap and a plug-lead spiral point tap are the same size and the same thread, and they are not interchangeable on the same hole.

By lead: how deep can it cut?

The lead is the tapered end of the tap, where the first few threads are progressively shallower. It exists so the tap can start in the hole. It also means the threads it cuts at that point are incomplete, so the usable thread ends before the tap does.

Tap	Lead length	Starts easily?	Usable thread near the bottom	Where it is used
Taper	Long — around 8 to 10 threads	Easiest	Very little	Starting a thread; followed by another tap
Plug	Moderate — around 3 to 5 threads	Yes	Most of the hole	General purpose; the usual choice
Bottoming	Short — around 1 to 2 threads	Difficult	Almost to the bottom	Finishing a blind hole after a plug tap

The practical consequences:

A taper tap needs the deepest hole and gives the shortest usable thread. It is the easiest to start and the hardest to use efficiently on its own — on a blind hole it leaves several millimetres of incomplete thread at the bottom.

A plug tap is the default. It starts readily, cuts usable thread through most of the hole, and handles the majority of work.

A bottoming tap cuts closest to the bottom, but is hard to start because there is almost no taper to guide it into the hole. It is normally run after a plug tap has already opened and aligned the thread, which means two operations rather than one.

That sequence — plug first, then bottoming — is the standard way to get a thread that runs to the bottom of a blind hole. It costs a second operation, which is why a drawing that requires full thread depth in a blind hole costs more than one that does not. The relationship between thread depth and drill depth is covered in the comparison of threaded hole depths.

By flute: which way do the chips go?

This is the difference that causes the most broken taps, and it is entirely about chip direction.

Tap	Chip direction	Suits	Does not suit
Straight flute	Chips stay in the flutes; must be reversed out	General work, through or blind	Deep holes; any job where clearing is difficult
Spiral point (gun)	Chips pushed forward, ahead of the tap	Through holes	Blind holes — chips pack at the bottom
Spiral flute	Chips pulled backwards, out of the hole	Blind holes	Weakest geometry; used with care

The rule is simple: on a blind hole, the chips have to come back out the way the tap went in. A spiral point tap pushes chips ahead of itself, which is excellent in a through hole where they exit the far side and disastrous in a blind hole where they have nowhere to go. They pack at the bottom, the effective hole shortens, torque climbs, and the tap breaks.

A straight flute tap is the general-purpose option. It cuts, the chips accumulate in the flutes, and the tap is reversed out of the hole periodically to clear them. It is the cheapest and most widely used, and on a shallow through hole it is entirely adequate. On a deep hole or a difficult material it means a lot of reversing.

A spiral flute tap has flutes ground at an angle that lifts the chips back up and out of the hole. That is exactly what a blind hole needs, and it is why this is the tap most often specified for blind-hole work. The trade is that the flute geometry leaves less material in the tap body, so it is more fragile than a spiral point tap and is run more carefully.

Form taps: no chips at all

There is a third family that sidesteps the chip problem completely.

A form tap — also called a thread forming tap or a fluteless tap — has no flutes and does not cut. It displaces material into the thread form, the way a thread rolling die forms a thread on a bolt. The material that would have become the chip instead becomes the thread.

Three consequences follow, and they are substantial.

There are no chips. Not fewer — none. That makes form tapping ideal for blind holes, for holes drilled downwards into a cavity, and for any orientation where clearing chips is awkward. It removes the entire failure mode described in the previous section.

The thread is stronger. Because the material flows into the thread form rather than being cut away, the grain follows the thread profile instead of being severed at every thread root. That is the same principle that makes rolled threads stronger than cut threads, and cold heading stronger than turning at a fillet — the grain running along the load path rather than across it.

The tap drill size changes. A cutting tap removes material, so the starting hole is sized for the minor diameter the thread will leave. A form tap displaces material, so the starting hole has to contain the volume that will be pushed into the thread — which means a larger tap drill than the same thread would use with a cutting tap. Form tap charts give the correct size, and using a cutting tap’s drill with a form tap will overload it.

The limitations are equally clear:

• The material has to be ductile enough to flow. Steels, stainless, copper alloys and many aluminium alloys form well. Cast iron will not — it is brittle and tears rather than deforming.
• The hole diameter is more critical, because there is less margin for error in the volume calculation.
• Hard materials are unsuitable, since the forming force rises sharply with hardness.

Where the material and the hole suit it, form tapping is often the better process on every measure — no chips, stronger thread, and a good surface finish on the flanks. Where it does not suit, it is not an option at all.

Hand taps and machine taps

Taps are also sold in hand and machine versions, and the difference is real even though they look similar.

Hand taps are designed to be turned by hand with a tap wrench. They are usually straight-fluted and come in sets of three — taper, plug and bottoming — so the thread can be started easily and finished to depth.

Machine taps are designed for power tapping on a machine, where the tap is held in a chuck or a floating holder and driven by the spindle. They are typically spiral point or spiral flute, because chip control is the whole problem when the tap is buried in a hole with no operator feel, and they are made to run at controlled speed and feed.

The distinction matters to a buyer in one practical way: the tap type affects whether a blind hole can be tapped at all, and therefore whether a drawing is feasible. A requirement for a thread right to the bottom of a small blind hole drives the process towards a bottoming tap after a plug tap, or towards thread milling, and both cost more than a thread that has a few millimetres of relief at the bottom.

Matching the tap to the material

Material behaviour decides most of the tap selection in practice.

Material	Behaviour at the tap	Usual approach
Aluminium	Cuts easily but galls and builds up on the flutes	Sharp tap, lubricant, spiral flute or form tap
Brass	Very easy; among the best materials to tap	Any tap type works; form taps are excellent
Free-cutting steel	Easy; short chips	Straight flute or spiral point
Medium carbon and alloy steel	Moderate	Spiral point for through holes, spiral flute for blind
Stainless steel	Work-hardens and galls; taps break readily	Sharp tap used once, lubricant, slightly larger drill, spiral flute or interrupted thread
Titanium	Tough and galls severely	Careful speeds, generous lubricant, or thread milling
Cast iron	Cuts as short chips; brittle	Cutting taps only; form taps will not work
Plastics	Easy to tap but threads are weak	Coarse threads, generous engagement, or inserts

Two general rules fall out of the table.

Hard and galling materials favour form tapping where they are ductile enough, because there is no chip to clear and no cutting edge to wear — but stainless sits awkwardly, since it forms well but the forming force is high.

Free-cutting grades make tapping dramatically easier. The same thread in 12L14 and in 304 stainless are not comparable operations; the first is routine, the second is where taps break. That is the same machinability argument that runs through every material comparison on this site.

Thread milling, and when to avoid the tap entirely

There is an alternative to tapping that removes the risk rather than managing it.

Thread milling cuts a thread with a small rotating cutter that follows a helical path, rather than with a tap. The advantages are significant on difficult work:

• One tool covers a range of thread sizes, because the diameter is set by the toolpath rather than by the cutter
• There is no tap to break in the hole, which is the single most expensive failure in tapping
• Chips are managed well, because the cutter is not buried in the material and the chips fall clear
• The thread can be cut to the bottom of a blind hole without a second operation, since the cutter can be fed on a controlled helix

The trade is speed: on a simple hole, tapping is faster. But on a large thread, a difficult material, a blind hole needing full depth, or a part that would be scrapped by a broken tap, thread milling is often the more economical route overall. It is run on the same CNC milling equipment that machines the rest of the part.

Why broken taps are the expensive failure

A broken tap is the worst common outcome in a machine shop, and it is worth understanding why, because it explains a lot of quoting behaviour.

The tap is harder than the part. Removing a broken tap from a hole — by spark erosion, by a tap extractor, or by annealing and drilling — is slow, uncertain, and often impossible without damaging the thread or the surrounding features. On a part that is already largely finished, a broken tap usually means scrapping the part and starting again.

Almost every broken tap traces back to one of four things:

• Wrong chip direction for the hole — a spiral point tap in a blind hole
• Insufficient drill depth, so the tap bottoms out on its lead before the thread is complete
• Work hardening, where the tap rubs rather than cuts and the material hardens against it
• A dull tap, reused past its life on a material that punishes it

All four are process decisions, and all four are made easier by a drawing that tells the shop what the thread has to do. Where a blind hole has a few millimetres of relief at the bottom, the whole problem becomes routine. Where it does not, the cost of achieving it is real, and it belongs in the quotation rather than in the scrap bin.

What to put on the drawing

Instead of	Write
M6 blind, full thread to the bottom	M6 — 6H — ⤓ 10 blind; state whether relief at the bottom is acceptable
Thread, depth not stated	The usable thread depth, and whether the hole is through or blind
Tap type specified on the drawing	Nothing — the tap follows from the hole, the material and the depth
Thread in stainless, no note	State the material; the tap and the drill allowance change
Thread in cast iron with a form tap in mind	Form tapping is not possible in brittle material
Deep small blind thread	Consider thread milling, or allow relief at the bottom

The one line that changes the most is whether relief is acceptable at the bottom of a blind thread. Where it is, the shop can use a plug tap, clear the chips, and produce the thread reliably. Where the thread genuinely has to run to the bottom, the operation changes — a second tap, a smaller drill allowance, possibly thread milling — and the price and the risk change with it.

Thread designations, classes and series are set out on the thread standards page, and the grades we run, with how each behaves at the tap, are on the materials page. Send the drawing with the material, the quantity and any tight requirement on thread depth or position, and the quote comes back within 24 hours with DFM feedback — including a note where a thread requirement is adding cost or risk that a small drawing change would remove. Orders start at 50 pieces per style and material, samples from a single piece in 5–10 days, and every batch ships with a material certificate (MTR) tracing the grade to its mill heat plus pre-shipment photos.

Taps make the hole; the screw that goes into it is a separate specification. A thread that gauges correctly in the hole can still fail at assembly if the external thread class does not match, which is why the drawing has to state the class on both parts. The external side of that conversation is covered in custom screw tolerance, and the parts themselves in custom screws.