Types of Taps: Taper, Plug, Bottoming, Spiral Point, Spiral Flute, and Forming Taps Explained
Every tap type exists to solve one of three problems: starting the thread, reaching the bottom of the hole, or getting the chips out. Here is how to match the tap to the hole, the material, and the machine.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 17 min read
On this page
Quick Answer
The main types of taps are defined by chamfer and flute geometry. Taper (7–10 chamfered threads), plug (3–5), and bottoming (1–2) taps are the three chamfer styles — plug is the general-purpose default, and blind holes are finished with a bottoming tap after a plug tap. Spiral point (gun) taps push chips forward and belong in through holes; spiral flute taps lift chips up and out and belong in blind holes. Forming taps make no chips at all, cold-forming threads in ductile materials like aluminum and brass. Pipe taps cut tapered NPT threads for pressure-tight seals. Match the tap to the hole type first, then to the material, then set speed and drill size — most broken taps are a chip-evacuation or tap-drill problem, not a bad tool.
Taper, Plug, and Bottoming Taps: It Is All in the Chamfer
Pick up any traditional hand tap set and you get three taps that look almost identical — because they are. The only difference between a taper, plug, and bottoming tap is the number of chamfered (tapered, incomplete) threads at the tip. The chamfer distributes the cutting work across several teeth: a long chamfer means each tooth removes a thin slice, which lowers torque and helps the tap start square; a short chamfer concentrates the cut but reaches full thread depth almost immediately.
The taper tap, with 7–10 chamfered threads, is the starter — easy to align, hard to overload, ideal for hand tapping and tough materials, but it cannot produce full threads near the bottom of a blind hole. The plug tap, with 3–5 chamfered threads, is the workhorse: it starts easily enough and threads deep enough that it is the default choice for most production tapping on CNC machines. The bottoming tap, with only 1–2 chamfered threads, is a finishing tool — you run it after a taper or plug tap when the drawing demands full threads close to the floor of a blind hole.
| Tap Type | Chamfered Threads | Cutting Load | Best Use |
|---|---|---|---|
| Taper (starter) tap | 7–10 | Lightest — load spread over the long chamfer | Starting threads square by hand; hard materials; through holes |
| Plug tap | 3–5 | Moderate | General-purpose and production CNC tapping; the default machine tap |
| Bottoming tap | 1–2 | Heaviest — nearly the full thread cut at once | Finishing full threads to the bottom of a blind hole, after a plug tap |
The classic blind-hole sequence is taper (or plug) first, bottoming second. Skipping the first tap and driving a bottoming tap straight into a drilled hole forces a few teeth to cut the entire thread at once — torque spikes and the tap snaps. Hole type drives every one of these decisions, so if the blind-versus-through distinction is not second nature yet, start with our guide to blind vs through holes before specifying thread depths.
Hand Taps vs Machine Taps, and Why Flute Geometry Decides Chip Direction
Hand taps are straight-flute HSS tools designed to be turned with a tap wrench — short forward turn, back off to break the chip, repeat. Machine taps are built for power-driven spindles on drill presses, lathes, and machining centers, and this is where flute geometry starts to matter, because a machine does not feel chips packing the way a hand operator does. A tap does not just cut a thread; it has to move every chip somewhere before the spindle reverses. Geometry determines where those chips go.
A spiral point tap — often called a gun tap — has an angular grind on the cutting face that shoots chips forward, ahead of the tap and out the open bottom of the hole. Its flutes are shallow, leaving a thick, rigid core, which makes it the strongest cutting tap and the fastest option for through holes. A spiral flute tap has helical flutes like a twist drill that lift chips up and out of the hole, auger-style. That lifting action is what keeps chips from packing into the bottom of blind holes, and it also handles the long, stringy chips from soft materials like aluminum, brass, and copper. Straight-flute taps remain the right call in short-chip materials like cast iron, where there is nothing stringy to evacuate.
| Tap Geometry | Chip Direction | Hole Type | Notes |
|---|---|---|---|
| Straight flute (hand tap) | Chips pack into the flutes | Shallow holes, cast iron and other short-chip materials | Simplest and cheapest; needs periodic reversal to break chips in deep holes |
| Spiral point (gun tap) | Pushes chips forward, ahead of the tap | Through holes | Strongest cutting tap — shallow flutes leave a solid core; fastest production option |
| Spiral flute | Lifts chips up and out of the hole | Blind holes | Helical flute acts like an auger; the standard choice for blind holes and stringy materials |
| Forming (fluteless) tap | No chips at all | Blind or through, ductile materials only | Cold-forms the thread; nothing to evacuate, nothing to jam |
The rule every shop floor learns once, the hard way: spiral point for through holes, spiral flute for blind holes. Running a spiral point tap into a blind hole rams chips into the hole bottom until torque spikes and the tap lets go — usually flush with the surface, where it is hardest to remove.
Forming Taps vs Cutting Taps: Chipless Threading
Everything above describes cutting taps — tools that machine the thread away and produce chips. A forming tap (also called a roll tap, fluteless tap, or cold-forming tap) has no cutting edges and no flutes. Instead, lobed threads on the tap displace the workpiece material, pressing it into the thread shape by plastic deformation. No material is removed, so no chips exist — nothing to evacuate, nothing to pack into a blind hole, nothing to bird-nest around the shank in stringy alloys.
The benefits compound. Formed threads are stronger than cut threads because the grain flow follows the thread contour instead of being severed, and the cold-working hardens the thread surface. Form taps themselves are stronger — a solid core with no flutes — and gauge beautifully over long production runs. The limitations are just as real: the material must be ductile enough to flow (aluminum, brass, copper, low-carbon steel, and many stainless grades qualify; cast iron and hardened steels do not), the tap drill must be larger and held to tighter size because the minor diameter is formed rather than cut, drive torque runs higher than a cutting tap of the same size, and lubrication is non-negotiable. Where those conditions are met, a forming tap is usually the fastest, cleanest, most reliable tapping process in the shop — and the single best upgrade for high-volume blind-hole work in aluminum.
Pipe Taps: NPT and Tapered Pipe Threads
Pipe taps are a category of their own because pipe threads are tapered. The North American standard is NPT (National Pipe Taper, defined by ASME B1.20.1): a 60° thread form cut on a 1:16 taper — 3/4 inch per foot — so the fitting wedges tighter with every turn and the thread flanks themselves form the pressure seal, assisted by PTFE tape or paste sealant. The dryseal variant NPTF is designed to seal at the roots and crests without sealant. British pipe threads (BSP/BSPT) use a 55° Whitworth form on the same 1:16 taper and are not interchangeable with NPT.
Tapping NPT differs from straight-thread work in ways that bite if you ignore them. Because the tap is tapered, it cuts along its entire engagement length, so torque requirements are far higher than a same-size straight tap — a 1/2-14 NPT tap is a serious workout even in aluminum. The drilled hole comes from a pipe tap drill chart, not the UNC chart (a 1/4-18 NPT thread starts from a 7/16" pilot hole), and some shops taper-ream before tapping to reduce cutting load. Depth control matters too: run the tap to the specified engagement, because an over-deep NPT thread leaves the fitting loose at the bottom of its travel. For the dimensional side — thread designations, TPI, pitch diameters, and tap drill sizes across metric, Unified, and pipe threads — our thread sizes and thread chart reference covers the tables.
Tap Materials and Coatings
Taps live a brutal life: they cut at low speed with huge contact area, then reverse under load. Substrate and coating choices follow directly from that. M2 high-speed steel is the general-purpose baseline — tough, affordable, and right for mild steel, aluminum, and brass. Cobalt HSS grades (M35, M42) add heat and wear resistance for stainless steel, alloy steels, and titanium, where M2 dulls fast. Solid carbide brings maximum wear resistance for abrasive materials like cast iron and high-silicon aluminum, but carbide is brittle — it belongs in rigid machines with rigid holders, never in a hand tap wrench or a wobbly drill press.
Coatings do two jobs: reduce friction and resist wear. Steam oxide is the humble classic — a porous black oxide surface that retains cutting oil and resists the galling that kills taps in stainless. TiN is the general-purpose gold coating for steels. TiCN is harder and more wear-resistant, a good match for abrasive and harder materials. TiAlN/AlTiN handles the highest cutting heat and suits faster, drier tapping. In soft aluminum, a bright (uncoated) polished tap often performs best because nothing on the surface encourages chip welding. Whatever the coating, it cannot rescue a wrong geometry or a wrong speed — coating is the last 20% of tap life, not the first 80%.
Tapping Speeds, Tap Drill Size, and How to Stop Breaking Taps
Tapping is one of the slowest operations in the shop for good reason: the tap is fully engaged on every flute, so heat and torque build fast. Cutting speed follows material hardness, and the ranges below are proven starting points for through-hole tapping with cutting oil — reduce roughly 25% for blind holes and for dry tapping, and start a new setup around 70% of the range.
| Workpiece Material | M2 HSS | M35 Cobalt HSS | Notes |
|---|---|---|---|
| Aluminum 6061 / 5052 | 20–40 m/min (66–131 SFM) | 25–50 m/min (82–164 SFM) | Runs fast but chips weld; rigid tapping and good lubricant; forming taps excel |
| Brass / bronze | 20–35 m/min (66–115 SFM) | 25–45 m/min (82–148 SFM) | Free-cutting; can often run with minimal coolant |
| Mild steel 1018 | 8–14 m/min (26–46 SFM) | 10–18 m/min (33–59 SFM) | The baseline ferrous material; cutting oil extends tap life |
| Alloy steel 4140 | 4–8 m/min (13–26 SFM) | 6–10 m/min (20–33 SFM) | Reduce speed for deep holes; watch torque as hardness climbs |
| Stainless 304 / 316 | 3–6 m/min (10–20 SFM) | 5–9 m/min (16–30 SFM) | Work-hardens if the tap dwells; keep the cut continuous, never rub |
| Titanium Grade 5 | Not recommended | 3–6 m/min (10–20 SFM) | Cobalt minimum, rigid setup, high-lubricity oil; Inconel slower still at 5–15 SFM |
| Grey cast iron | 8–14 m/min (26–46 SFM) | 10–18 m/min (33–59 SFM) | Short chips suit straight-flute taps; abrasive — coated or carbide taps last longer |
The tap drill size deserves equal attention. Standard tap drill charts target about 75% thread engagement — and that is deliberate, not a compromise. Driving the drill size down toward 100% engagement roughly triples tapping torque for a marginal gain in thread strength, and it is a leading cause of snapped taps. A 75% thread in a properly sized hole is stronger than the bolt that goes into it in most applications. Remember also that a chamfer before tapping pays twice: it removes the burr that would otherwise tear on the first thread and it guides the tap square into the hole — the same countersink operation covered in our countersink holes guide. Thread fit callouts (2B/6H internal classes) belong to the broader tolerance system; our CNC machining tolerances guide explains how to specify them sensibly.
Put the causes of tap breakage in order and they read: wrong tap drill size, chips packed in a blind hole, misalignment, too much speed, too little lubricant, bottoming out. Rigid tapping — where the CNC synchronizes spindle rotation and Z feed to the thread pitch — fixes the alignment and feed errors; a floating or tension-compression holder absorbs mismatch on older machines. Peck-tap deep holes in tough materials. And when a tap does break, stop: do not drive a second tap into the hole. Removal means EDM, a tap extractor, or careful carbide-drill surgery — all slower than doing it right the first time.
FAQ: Types of Taps
What are the three main types of hand taps?
The three classic hand taps are taper, plug, and bottoming, and the only difference between them is the chamfer length at the tip. A taper tap has 7–10 chamfered threads, so it starts easily and stays square — it is the starter tap. A plug tap has 3–5 chamfered threads and is the general-purpose choice for most holes. A bottoming tap has only 1–2 chamfered threads and cuts full-depth thread almost to the floor of a blind hole. In a traditional hand-tapping kit you start with the taper, follow with the plug, and finish blind holes with the bottoming tap.
Which tap should I use for a blind hole?
For a blind hole, use a spiral flute tap — its helical flutes lift chips up and out of the hole the way an auger clears a drilled hole, which prevents the chip packing that snaps taps at the bottom. Choose a plug chamfer (3–5 threads) for the main threading, and follow with a bottoming tap only if the drawing requires full threads closer to the hole floor. Drill the hole deeper than the required thread by several pitches to leave room for chips and the tap chamfer. In ductile materials like aluminum, a forming tap is an even safer blind-hole option because it produces no chips at all.
What is the difference between spiral point and spiral flute taps?
The difference is the direction each one moves chips. A spiral point tap — also called a gun tap — has angular cutting faces that shoot chips forward, ahead of the tap and out the bottom of the hole. That makes it the right choice for through holes, and its shallow flutes leave a strong, rigid core. A spiral flute tap has helical flutes like a drill, which pull chips backward up out of the hole, making it the standard choice for blind holes where forward chips would pack into the bottom. Using a spiral point tap in a blind hole is one of the most common causes of broken taps.
When should I use a forming tap instead of a cutting tap?
Use a forming tap when the workpiece material is ductile — aluminum, brass, copper, low-carbon steel, and many stainless grades — and you want chipless threading, especially in blind holes. Forming taps displace material by cold forming rather than cutting it, so there are no chips to pack, jam, or bird-nest, and the threads come out stronger because the grain flow follows the thread contour. The trade-offs: they need a larger, more accurately sized tap drill, roughly higher drive torque, generous lubrication, and a material with enough ductility to flow. Brittle materials like cast iron must be cut, not formed.
What causes taps to break, and how do I prevent it?
Most broken taps trace back to a short list: a tap drill that is too small, which drives torque up; chips packing into a blind hole; misalignment between tap and hole; running too fast or without lubricant; and the tap hitting the hole bottom. Prevention follows the same list — drill to the correct size for about 75% thread engagement, match the tap geometry to the hole (spiral point for through, spiral flute for blind), use rigid tapping or a quality tension-compression holder, apply proper cutting oil, leave chip clearance at the bottom of blind holes, and slow down in stainless, titanium, and other difficult alloys.
What is a pipe tap, and how is it different from a regular tap?
A pipe tap cuts pipe threads — most commonly NPT in North America — which are tapered rather than straight. NPT threads have a 60° thread form and a 1:16 taper (3/4 inch per foot), so the fitting wedges tighter as it is threaded in and the thread flanks themselves create the pressure seal, usually with tape or paste sealant. Because the tap is tapered, it cuts along its whole length and requires much more torque than a straight tap of similar size, and the drilled hole must match the pipe tap drill chart, not the standard UNC chart. BSP pipe taps use a 55° form and are not interchangeable with NPT.
Related Resources
CNC Machining Surface Finish: The Ra Chart, Explained
The CNC machining surface finish chart: Ra values in μm and μin, N1–N12 grades, what each process achieves, what…
Passivation of Stainless Steel: Process, Specs, and When Parts Need It
Passivation of stainless steel explained for machined parts: the chemistry, ASTM A967 and AMS 2700 methods, nitric…
GD&T Basics for CNC Machined Parts: The Symbols That Matter
GD&T basics for machined parts: the 14 symbols explained, feature control frames, datums, MMC bonus tolerance, true…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Tapped Holes on Your Drawing? Send It Over.
IsoCNC machines internal and external threads — metric, UNC/UNF, and NPT — in aluminum, steel, stainless, titanium, brass, and engineering plastics, with thread gauges and inspection reports on every lot. Not sure whether your blind holes need spiral flute or forming taps, or whether your thread spec is driving cost? An engineer reviews every RFQ, typically within 1–2 business days.