# Types of taps and how to tap a hole

Short answer: The main types of taps are taper (7 to 10 chamfered threads), plug (3 to 5) and bottoming (1 to 2). Spiral point taps push chips forward for through holes; spiral flute taps lift chips out of blind holes. Form taps make no chips and need a larger drill: about 5.6 mm for M6 instead of 5 mm.

## Key takeaways

- Taper taps have 7 to 10 chamfered threads, plug taps 3 to 5 and bottoming taps 1 to 2.
- Spiral point (gun) taps are for through holes; spiral flute taps are for blind holes.
- Form tap drill = D minus 0.0068 times percent thread divided by TPI; M6 needs about 5.6 mm.
- Cobalt (HSS-E) taps suit stainless steel; carbide taps need a rigid CNC machine.
- Drill blind holes deeper than the thread by the chamfer length plus about two pitches.

## Types of taps: the short version

A tap cuts or forms an internal thread in a drilled hole. The types of taps differ in three ways: the chamfer at the tip (taper, plug or bottoming), the flute shape that handles chips (straight flute, spiral point or spiral flute), and whether the tap cuts the thread or forms it without chips.

| Tap type | How it handles chips | Best for |
|---|---|---|
| Straight flute (hand tap) | Chips stay in the flutes; reverse to break them | Hand tapping, cast iron, brass, short-chipping materials |
| Spiral point (gun tap) | Pushes chips ahead of the tap, out the bottom | Through holes in steel, stainless and aluminum, machine tapping |
| Spiral flute | Pulls chips up and out of the hole | Blind holes, stringy chips, machine tapping |
| Thread forming (roll) tap | Makes no chips; displaces metal | Ductile metals: aluminum, copper, mild and stainless steel |
| Combination drill and tap | Drill point, then a short spiral point tap | Thin sheet and through holes with a hand drill |

Every tap needs the right hole first. For cutting taps, the hole is the [tap drill size](https://machinistcharts.com/tap-drill/); for form taps it is larger, as shown in the form tap drill chart below. Pick the thread from the [thread pitch chart](https://machinistcharts.com/guides/thread-pitch-chart/) before picking a tap.

## Taper, plug and bottoming taps

Taper, plug and bottoming taps differ only in chamfer length: a taper tap has 7 to 10 chamfered threads, a plug tap 3 to 5 and a bottoming tap 1 to 2, per ASME B94.9. The chamfer spreads the cutting load over several teeth, so a longer chamfer starts more easily but leaves more incomplete thread at the bottom of a hole.

| Tap | Chamfered threads | Incomplete length on M8 × 1.25 (mm) | Use |
|---|---|---|---|
| Taper | 7 to 10 | 8.75 to 12.5 | Easiest start; through holes; hard materials by hand |
| Plug | 3 to 5 | 3.75 to 6.25 | The general-purpose tap; through holes and blind holes with room below |
| Semi-bottoming | 2 to 3 | 2.5 to 3.75 | Blind holes on machine taps |
| Bottoming | 1 to 2 | 1.25 to 2.5 | Finishing a blind hole to near full depth after a plug tap |

A common three-tap hand set holds one of each. For a through hole, a plug tap alone is usually enough. For a blind hole that must be threaded close to the bottom, start with a taper or plug tap and finish with a bottoming tap. A bottoming tap used alone is hard to start straight and loads its few cutting teeth heavily.

European taps describe the same thing with chamfer form letters per DIN 2197. Form C, with 2 to 3 chamfered threads, is the usual chamfer on spiral flute taps for blind holes.

## Spiral point vs spiral flute vs straight flute taps

Use a spiral point tap for through holes and a spiral flute tap for blind holes. A spiral point tap, also called a gun tap, has a ground angle at the front of the flutes that shoots chips forward, out the bottom of the hole. A spiral flute tap has helical flutes, like a drill, that lift chips up and out the top.

### Spiral point (gun) taps

Spiral point taps have shallow flutes and a strong core, so they take higher speeds and break less often than other cutting taps. The chips never pass back over the cutting edges, so the tap can run in one direction from start to finish without reversing to break chips. Do not use one in a blind hole: chips pack ahead of it and the tap breaks when they fill the bottom.

### Spiral flute taps

Spiral flute taps are made for blind holes in materials that make long, stringy chips, such as aluminum, mild steel and stainless steel. A higher helix angle lifts chips better in soft materials; a lower helix gives a stronger tap for tough steels. The deeper flutes mean a weaker tap than a spiral point of the same size.

### Straight flute (hand) taps

Straight flute taps are the classic hand taps. Chips stay in the flutes, so the tap must be reversed every turn or so to break them. They work best in cast iron, brass and other materials that make short, broken chips, and they are the most common taps in hand tap sets.

## Thread forming taps and form tap drill chart

A thread forming tap, also called a roll tap or form tap, has no cutting edges. It presses the thread into the hole wall by cold-forming the metal, so it makes no chips and needs a larger drill than a cutting tap. A common formula, used by tap makers, is drill = D − (0.0068 × % thread) / TPI for inch threads, or D − 0.0068 × % thread × P in mm.

At 65 % thread, a typical target for form tapping, the metric rule reduces to drill ≈ D − 0.44 × P. The shortcut D − 0.5 × P gives about 74 % thread, which is on the tight side and raises tapping torque. The tables below apply the 65 % formula and pick the nearest stock drill. Tap makers publish their own recommended holes; their chart wins, and the hole should be checked with a pin gauge in production.
[](https://machinistcharts.com/tap-drill/m2/)[](https://machinistcharts.com/tap-drill/m2-5/)[](https://machinistcharts.com/tap-drill/m3/)[](https://machinistcharts.com/tap-drill/m3-5/)[](https://machinistcharts.com/tap-drill/m4/)[](https://machinistcharts.com/tap-drill/m5/)[](https://machinistcharts.com/tap-drill/m6/)[](https://machinistcharts.com/tap-drill/m8/)[](https://machinistcharts.com/tap-drill/m10/)[](https://machinistcharts.com/tap-drill/m12/)[](https://machinistcharts.com/tap-drill/m14/)[](https://machinistcharts.com/tap-drill/m16/)[](https://machinistcharts.com/tap-drill/m18/)[](https://machinistcharts.com/tap-drill/m20/)

| Thread | Pitch mm | Calculated hole mm | Form tap drill mm | Thread % with that drill | Cutting tap drill mm (for comparison) |
|---|---|---|---|---|---|
| M2 | 0.4 | 1.823 | 1.8 | 74 | 1.6 |
| M2.5 | 0.45 | 2.301 | 2.3 | 65 | 2.05 |
| M3 | 0.5 | 2.779 | 2.8 | 59 | 2.5 |
| M3.5 | 0.6 | 3.235 | 3.2 | 74 | 2.9 |
| M4 | 0.7 | 3.691 | 3.7 | 63 | 3.3 |
| M5 | 0.8 | 4.646 | 4.6 | 74 | 4.2 |
| M6 | 1 | 5.558 | 5.6 | 59 | 5 |
| M8 | 1.25 | 7.447 | 7.4 | 71 | 6.8 |
| M10 | 1.5 | 9.337 | 9.3 | 69 | 8.5 |
| M12 | 1.75 | 11.226 | 11.2 | 67 | 10.2 |
| M14 | 2 | 13.116 | 13.1 | 66 | 12 |
| M16 | 2 | 15.116 | 15.1 | 66 | 14 |
| M18 | 2.5 | 16.895 | 16.9 | 65 | 15.5 |
| M20 | 2.5 | 18.895 | 18.9 | 65 | 17.5 |

[](https://machinistcharts.com/tap-drill/2-56/)[](https://machinistcharts.com/drill-size/5-64-inch/)[](https://machinistcharts.com/tap-drill/4-40/)[](https://machinistcharts.com/drill-size/number-38/)[](https://machinistcharts.com/tap-drill/6-32/)[](https://machinistcharts.com/drill-size/1-8-inch/)[](https://machinistcharts.com/tap-drill/8-32/)[](https://machinistcharts.com/drill-size/number-25/)[](https://machinistcharts.com/tap-drill/10-24/)[](https://machinistcharts.com/drill-size/11-64-inch/)[](https://machinistcharts.com/tap-drill/1-4-20/)[](https://machinistcharts.com/drill-size/number-1/)[](https://machinistcharts.com/tap-drill/5-16-18/)[](https://machinistcharts.com/drill-size/letter-l/)[](https://machinistcharts.com/tap-drill/3-8-16/)[](https://machinistcharts.com/drill-size/letter-s/)[](https://machinistcharts.com/tap-drill/1-2-13/)[](https://machinistcharts.com/drill-size/15-32-inch/)[](https://machinistcharts.com/tap-drill/10-32/)[](https://machinistcharts.com/drill-size/number-16/)[](https://machinistcharts.com/tap-drill/1-4-28/)[](https://machinistcharts.com/drill-size/15-64-inch/)

| Thread | Calculated hole in | Form tap drill | Thread % with that drill | Cutting tap drill (for comparison) |
|---|---|---|---|---|
| #2-56 | 0.0781 | 5/64" (0.0781) | 65 | #50 (0.0700) |
| #4-40 | 0.1009 | #38 (0.1015) | 62 | #43 (0.0890) |
| #6-32 | 0.1242 | 1/8" (0.1250) | 61 | #36 (0.1065) |
| #8-32 | 0.1502 | #25 (0.1495) | 68 | #29 (0.1360) |
| #10-24 | 0.1716 | 11/64" (0.1719) | 64 | #25 (0.1495) |
| 1/4-20 | 0.2279 | #1 (0.2280) | 65 | #7 (0.2010) |
| 5/16-18 | 0.2879 | L (0.2900) | 60 | F (0.2570) |
| 3/8-16 | 0.3474 | S (0.3480) | 64 | 5/16 (0.3125) |
| 1/2-13 | 0.4660 | 15/32" (0.4688) | 60 | 27/64 (0.4219) |
| #10-32 | 0.1762 | #16 (0.1770) | 61 | #21 (0.1590) |
| 1/4-28 | 0.2342 | 15/64" (0.2344) | 64 | #3 (0.2130) |

- **Where form taps work:** ductile materials, such as aluminum, copper, zinc die castings, mild steel and austenitic stainless steel. The formed thread is often stronger than a cut thread because the grain is not cut.

- **Where they do not:** brittle materials such as gray cast iron, and very hard steels.

- **Lubrication matters more:** form taps need a good lubricant; many have small oil grooves on the side for it.

- **The crest is not flat:** a formed thread has a small split at the crest of the minor diameter. That is normal; check the thread with a go/no-go gauge, not by eye.

Drilling a form tap hole to the cutting tap size is the most common way to break a form tap. A 1/4-20 form tap needs about a #1 drill, not the #7 used for cutting. The 4-40 form tap drill works out to #38 and the 10-32 to #16.

## Tap materials, hand taps and machine taps

Most taps are high-speed steel (HSS). Cobalt HSS (HSS-E) taps last longer in stainless steel and tough alloy steels. Carbide taps are for rigid CNC machines tapping cast iron, aluminum alloys and hardened steel at high volume; they are brittle and break if tapped by hand.

- **HSS:** the default for hand taps and general machine tapping, usually M2 or a similar [molybdenum high-speed steel](https://machinistcharts.com/material/m2-high-speed-steel/).

- **HSS-E (cobalt):** high-speed steel with about 5 % to 8 % cobalt, such as M35 or M42. It holds its hardness at higher cutting temperature, which helps in [304 stainless](https://machinistcharts.com/material/304-stainless/) and other work-hardening materials.

- **Powder metallurgy HSS (PM-HSS):** a finer, more uniform structure than conventional HSS, for longer life in machine tapping.

- **Carbide:** highest speed and wear life, lowest toughness. Only for machines with rigid tapping or a good tapping head.

- **Coatings:** steam oxide (black) helps hold lubricant and reduces galling in steel; TiN and TiCN add wear resistance. Uncoated bright taps are often preferred for aluminum, where coatings can let material build up.

### Hand taps and tap sets

A hand tap has a square drive on the shank and is turned with a tap wrench (the hand tap tool) or a T-handle for small sizes. A basic tap set holds taps, matching tap drills and a wrench; a metric set covers sizes such as [M3](https://machinistcharts.com/tap-drill/m3/), [M4](https://machinistcharts.com/tap-drill/m4/), [M5](https://machinistcharts.com/tap-drill/m5/), [M6](https://machinistcharts.com/tap-drill/m6/) and [M8](https://machinistcharts.com/tap-drill/m8/); an inch set covers [6-32](https://machinistcharts.com/tap-drill/6-32/), [8-32](https://machinistcharts.com/tap-drill/8-32/), [10-24](https://machinistcharts.com/tap-drill/10-24/), 10-32 and [1/4-20](https://machinistcharts.com/tap-drill/1-4-20/). A "tap bit" usually means a tap with a 1/4 in hex shank for a drill driver; it is only suited to small through holes in thin material.

### Machine taps and tolerance marks

Machine taps are spiral point, spiral flute or form taps made for a drill press, tapping head or CNC spindle, often with a reduced neck and a specific geometry for one material group. Tap size tolerance is marked on the shank: metric taps by class, such as ISO 2 (6H), the standard for general nut threads; inch taps by H limit. An H limit gives the pitch diameter oversize in steps of 0.0005 in: H1 is basic to +0.0005 in, H2 is +0.0005 to +0.0010 in, H3 is +0.0010 to +0.0015 in. See [thread classes and fits](https://machinistcharts.com/guides/thread-classes-and-fits/) for what the classes mean.

## How to tap a hole, step by step

To tap a hole: drill the correct tap drill, chamfer the hole, start the tap square, use cutting fluid, and turn forward with regular reversals to break the chip. In detail:

1. **Pick the drill.** Look up the tap drill for the thread, for example [M6](https://machinistcharts.com/tap-drill/m6/) (5 mm, about 77 % thread) or [1/4-20](https://machinistcharts.com/tap-drill/1-4-20/) (#7, about 75 % thread). In stainless or hard steel, a slightly larger drill lowers the torque: M6 with a 5.1 mm drill gives about 69 % thread. Check any drill with the [thread percentage calculator](https://machinistcharts.com/calculators/thread-percentage/).

2. **Spot and drill.** Center or spot drill, then drill to size. For a blind hole, drill deeper than the thread (see below).

3. **Chamfer the hole.** Countersink the mouth to just over the thread's major diameter, 90° for most work. It helps the tap start and stops the first thread from raising a burr.

4. **Align the tap.** Start the tap square to the surface. On a drill press or mill, hold the tap in the chuck or use a spring-loaded tap guide and turn the spindle by hand. By hand, check squareness with a small square from two directions after the first turn.

5. **Apply cutting fluid.** Use tapping fluid or sulfurized cutting oil on steel and stainless, a fluid made for aluminum on aluminum, and little or none on cast iron and brass.

6. **Turn and break the chip.** With a straight flute hand tap, turn forward a half to one turn, then back a quarter to a half turn to break the chip. Spiral point and form taps do not need reversing.

7. **Clear chips and finish.** In a blind hole, back the tap out, blow or brush the chips out, and continue. Switch to a bottoming tap for the last threads. Stop as soon as resistance rises sharply; that is the bottom.

8. **Check the thread.** Use a go/no-go plug gauge or the mating screw. Clean the thread and deburr the mouth.

### How deep to drill a blind hole for tapping

Drill a blind hole deeper than the required thread by at least the tap's chamfer length plus room for chips. A working rule is thread depth + chamfer threads × P + 2 × P, measured to the full drill diameter, plus the drill point (about 0.3 × D for a 118° point). The table uses a plug tap with 5 chamfered threads and a thread depth of 1.5 × D:
[](https://machinistcharts.com/tap-drill/m6/)[](https://machinistcharts.com/tap-drill/m8/)[](https://machinistcharts.com/tap-drill/m10/)

| Thread | Thread depth (1.5 × D) mm | Plug chamfer (5 P) mm | Chip room (2 P) mm | Full-diameter drill depth mm | Depth to drill point (118°) mm |
|---|---|---|---|---|---|
| M6 | 9 | 5 | 2 | 16 | 17.5 |
| M8 | 12 | 6.25 | 2.5 | 20.75 | 22.8 |
| M10 | 15 | 7.5 | 3 | 25.5 | 28.1 |

A bottoming tap shortens the chamfer allowance to 1 or 2 pitches. A thread depth of 1.5 × D is generous in steel; the guide to [thread engagement length](https://machinistcharts.com/guides/thread-engagement-length/) shows what each material really needs.

## How to avoid a broken tap

Most taps break from one of four causes: a hole that is too small, a tap that is not square, chips packed in the flutes or the bottom of a blind hole, or a dull tap. Each has a simple fix.

- **Use the right drill.** Never use the cutting tap drill for a form tap. In tough material, choose a drill that gives 60 % to 65 % thread rather than 75 %.

- **Keep it square.** Use a tap guide or the machine spindle. A tap pushed sideways snaps at the shank or the first full thread.

- **Clear chips.** Reverse straight flute taps often, use spiral flute taps in blind holes, and never let a spiral point tap run into a blind hole.

- **Do not bottom out.** Mark the tap or set a depth stop so it stops before the hole bottom.

- **Replace worn taps.** A dull tap needs more torque and tears the thread. Rising torque on a tap that used to cut freely is the sign.

- **Do not force it by hand.** Below about M3 or #4, use a small T-handle and a light touch; a long tap wrench gives too much leverage to feel the tap.

> A broken HSS tap is harder than any drill. Remove it with a tap extractor that fits into the flutes, by spark erosion (EDM), or, in an aluminum part, by dissolving the steel in a hot alum solution. Do not try to drill it out with an ordinary drill; that usually ruins the hole.

After tapping, use the right torque for the screw: the [bolt torque chart](https://machinistcharts.com/bolt-torque/) and the [bolt torque calculator](https://machinistcharts.com/calculators/bolt-torque/) give values by size and grade.

## Common questions

### What is the difference between taper, plug and bottoming taps?

Only the chamfer at the tip differs. A taper tap has 7 to 10 chamfered threads and starts most easily. A plug tap has 3 to 5 and is the general-purpose tap. A bottoming tap has 1 to 2 and threads close to the bottom of a blind hole, usually after a plug tap.

### Spiral point or spiral flute tap: which should I use?

Use a spiral point (gun) tap for through holes: it pushes chips ahead, out the bottom. Use a spiral flute tap for blind holes: it lifts chips up and out of the hole. A spiral point tap in a blind hole packs chips at the bottom and can break.

### What size drill for a form tap?

A form tap needs a larger hole than a cutting tap. A common formula is drill = D minus 0.0068 times percent thread divided by TPI. At 65 percent thread, M6 needs about 5.6 mm, M8 about 7.4 mm and 1/4-20 about a #1 drill (0.2280 in). Check the tap maker's chart.

### What is the 4-40 form tap drill size?

For a 4-40 thread forming tap, the 65 percent formula gives a hole of about 0.1009 in, which is a #38 drill (0.1015 in). The cutting tap drill for 4-40 is a #43 (0.0890 in); using it with a form tap risks breaking the tap.

### Can you use a form tap in cast iron?

No. Thread forming taps need a ductile material that flows, such as aluminum, copper, mild steel or austenitic stainless steel. Gray cast iron is brittle and crumbles instead of forming. Use a straight flute or spiral point cutting tap in cast iron, usually dry.

### How do you keep a tap from breaking?

Use the correct drill size, start the tap square with a tap guide, use cutting fluid, and reverse a straight flute hand tap a quarter to half turn after every half to full turn to break the chip. Never bottom out the tap in a blind hole, and replace dull taps.

### Are cobalt taps better than HSS taps?

Cobalt (HSS-E) taps with about 5 to 8 percent cobalt, such as M35 or M42, keep their hardness at higher temperatures and last longer in stainless steel and tough alloy steels. For aluminum, brass and mild steel, standard HSS taps work well and cost less.

Source page: https://machinistcharts.com/guides/types-of-taps/
Updated: 2026-10-24
Publisher: MachinistCharts (https://machinistcharts.com)
