The Different Types of Taps

Thursday, 4 March 2021  |  Admin

The Different Types of Taps

HAND TAPS ISO 529

These are straight flute general purpose tools which can be used for both machine or hand tapping. They are generally the most economical tool for use on production runs, but are best on materials that produce chips, or where the swarf breaks readily. Where deep holes are to be tapped, in materials which produce stringy swarf, serial taps may be needed, especially for coarse threads.

ISO 529 hand taps can be supplied in sets of three; bottom, second and taper leads, or individually.

BOTTOM TAPS have a chamfer (lead) of 1–2 threads, the angle of the lead being around 18 degrees per side. They are used to produce threads close to the bottom of blind holes. 

SECOND TAPS have a lead of 3-5 threads at 8 degrees per side. They are the most popular and can be used for through holes, or blind holes where the thread does not need to go right to the bottom.

TAPER TAPS have a lead of 7-10 threads at 5 degrees per side. The taper lead distributes the cutting force over a large area, and the taper shape helps the thread to start. They can therefore be used to start a thread prior to use of second or bottom leads, or for through holes.

IMPORTANT NOTE ON TERMINOLOGY!  In the UK, bottom taps are often referred to as ‘plugs’. In North America second taps are often referred to as ‘plugs’. This can easily lead to confusion. To avoid problems when ordering it is best to use the terms bottom, second and taper.

Another variation is that second taps are sometimes referred to as ‘intermediate’, and taper taps can be called ‘firsts’.

SERIAL TAPS DIN 352

As a rule of thumb ISO 529 taps should not be used to produce threads longer than 1.5 times the tap diameter as breakages may occur. For deeper holes and in tougher or difficult to work materials serial taps can be used.

Serial taps come in sets of three and have leads similar to ISO 529 taps. They are however graduated in diameter so that the first tap used, recognised by one groove on the shank, is smaller than the second which has two grooves. The required thread diameter is achieved by the finishing tap, no grooves. The material is therefore removed in stages so that there is less stress generated than with ISO 529 taps. The disadvantage of these taps is the longer time taken to produce a thread.

MACHINE TAPS

Machine taps are so called because they are designed to be run at higher speeds, and need less cutting power than hand taps.

SPIRAL POINT  Also known as ‘gun nose’ or ‘bull nose’ or chip driver. These taps are dimensionally the same as a hand tap, second lead, but have the cutting face ground back relative to the axis of the tap, for the lead portion. This gives the flute a better cutting action, requiring less power, and pushes the cut material forward, allowing free flow of coolant along the flutes to the cutting edge. The flutes are not ground as deeply as for hand taps, giving the tap greater strength. It can therefore be run at higher speeds.

Spiral point taps are ideal for machine tapping of through holes, or blind holes where there is enough clearance beyond the threaded portion to accommodate the swarf.

SPIRAL FLUTE  These taps are used to produce a thread close to the bottom of a blind hole and therefore have a very short lead. The right hand spiral cut of the flutes acts to force the swarf away from the cutting teeth to the rear of the flutes and out of the hole. They are better on materials which form long continuous stringy swarf, rather than chips. They are also better to tap a thread in a hole where there is a break in the material, e.g. another hole, as the spiral fluting helps the tap to pick up on the other side.

Spiral flute taps can have slow or fast helix angles. Slow spirals are used for non ferrous materials, and fast spirals for most other materials. We supply fast spiral as standard.

FLUTELESS  Otherwise known as ‘Roll’, ‘Forming’ or Polygon taps. Used for the chipless production of threads in ductile materials such as copper, aluminium or soft brass. As the name implies they do not have flutes but lobes, which contact the work piece to form the thread by extrusion. They are operated at high speeds and are better at maintaining size. As long as all of the correct operating criteria are met, i.e. speed, hole size and lubrication, they have a longer lif e and less breakages than with other types of machine taps. Because they produce no chips they are very suitable for blind hole tapping.

Fluteless taps require different tapping drill sizes and higher operating speeds than conventional taps, see later. The y also produce stronger threads.

LONG SHANK TAPS

MACHINE NUT (BS949)  These taps were designed for tapping nuts on machines, and have a long thread, shank and square length. The shank diameter is reduced below the thread minor diameter to enable the tap to run through the work piece. This was originally to allow nuts to collect on the shank. For nut production, taper leads were used to distribute the cutting action, but these taps are now generally used as long reach, and are supplied also in bottom and second leads.

DIN 376 and 374  These are European standard taps that are dimensionally different to the standard ISO 529 UK types. They are generally longer and have reduced shanks as do Nut Taps.

Basically DIN 376 are for standard coarse threads, and DIN 374 for fine threads. A third type DIN 371 is available. These have bigger shanks, so are not really classed as long reach. All of these taps are available in the same types as ISO 529, se e previous pages.

DIN 376 STRAIGHT FLUTE

DIN 376 SPIRAL POINT

DIN 376 SPIRAL FLUTE

 

PIPE TAPS

We supply BSP, BSPT to BS 949.9 and ANP taps to BS 949.3. See tap dimensions sheets.

OTHER TYPES

There are many other types of tap available, such as interrupted thread, series, tandem etc, but these are normally fo r special applications. We would advise you on enquiry should you require anything other than the standard forms listed here. We do stock some taps other than normal standards, as you can see below:-

TRAPEZOIDAL TAP

SURFACE COATINGS

While selecting the correct type of tap for a job, the material to be tapped should also be considered. This may determine the surface coating that should be applied to the tap in order to extend its life.

Most taps are supplied with no surface treatment. They are referred to as ‘Bright Finish’. These taps are mainly for use on non-ferrous materials, or steels that do not cold weld. Bright finish taps are therefore suitable for all hand operations, where speeds are too low for cold welding to occur, and for most machine operations.

STEAM TEMPERING & NITRIDING.

Nitriding hardens the tap’s surface skin and gives a grey/black appearance. It extends tap life when used on abrasive materials such as Copper, Aluminium alloys and Plastics, but it can make the tap brittle and more prone to breakage. Steam Tempering gives a blue/black finish. It causes minute imperfections on the surface of the tap. These cause the tapping lubricant to be retained more readily, reducing friction and the possibility of cold welding. This helps the tap to cope with both mild and stainless steels.

Both above processes are normally only required for Spiral point and Spiral flute taps when the work piece material requires them. These taps are known as ‘Steam tempered and nitrided’ and have a blue/black finish.

TITANIUM NITRIDE (Tin)  This is a gold coloured coating only a few microns thick which is not metallic so reduces the chance of cold welding. It is applied by vapour deposition using special purpose machines. It imparts to the tool a surface hardness of around 80-85 Rockwell. It also imparts a good abrasive resistance and subsequent decrease in friction between the tool and the work piece. This can allow tapping at higher speeds. Suitable for most stainless steels.

The process can increase the price of a tap significantly. When the tap is reground the coating will be removed. This coating is more appropriate to Fluteless taps than steam tempering and nitriding.

TITANIUM CARBIDE NITRIDING (TiCn)  This coating is applied to the tool in the same way as Tin, and gives a silver/grey finish. It has the same qualities as Tin coating, but more so. It is equally more expensive. Suitable for very abrasive and high tensile materials.

SPEEDS, FEEDS AND LUBRICANTS

Tapping speeds are determined by many factors. The main ones are:-

  • Thread pitch 
  • Material being tapped
  • Hole depth
  • Hole type, through or blind e) Depth of thread
  • Lubricant quality and flow rate

Tapping speeds can be calculated using:-   

RPM = Feed speed (SFM)
      0.26 x Tap OD

Recommended SFM are given later.

Tapping speeds should be decreased if :-

  • Lubricant is poor, or flow is restricted
  • Bottom lead or Spiral flute taps are used
  • Thread depth (%) increases.
  • Thread pitch is coarse
  • Cutting taper threads (50% normal speed)
  • Cutting Acme or Trapezoidal threads (40% normal speed)

Tapping speeds can be increased if:-

  • Thread depth decreases
  • Thread pitch is fine
  • Coolant flow and quality is good
  • Spiral point taps are used

RECOMMENDED FEED SPEEDS AND LUBRICANTS

Speeds given are for machine tapping using HSS taps, and are given in feet per minute

MATERIAL 

FEED SPEED (SFM) 

LUBRICANT

Aluminium

70-90

Soluble oil

Aluminium alloy

50-70

Soluble, light base or lard oil

Brass

60-100

Light base oil

Bronze

30-40

Light base oil

Copper

60-80

Light base oil

Gun metal

50-60

Soluble, light base or lard oil

Grey cast iron

30-60

Dry or soluble oil

Alloy cast iron

15-30

Sulphur based oil

Malleable iron

20-40

Soluble or sulphur based oil

Magnesium alloy

50-70

Soluble oil or paraffin with lard oil

Nimonic alloy

10-12

Very high pressure cutting oil

Plastics

50-70

Dry, freeze spray, liquid soap

Mild steel

30-50

Sulphur based oil

Carbon steel to 4% 

20-40

Sulphur based oil

Carbon steel to 7%

20-30

Sulphur based oil

Carbon steel 7%+

15-25

Sulphur based oil

Steel alloys to 60T

15-25

Sulphur based oil

Steel alloys 60T+

10-15

Sulphur based oil

Stainless steels

10-20

Sulphur based oil

Tool steels

15-25

Sulphur based oil

With so many variables affecting tapping speeds there may need to be some experimentation to find the ideal. A good rule is to start at the slowest speed and work up.

 

TROUBLESHOOTING

Many factors can affect the quality of a tapped thread. Some more common problems are listed along with probable causes.

POOR THREAD FINISH 

  • Misalignment of tap and work piece
  • Incorrect feed rate
  • Chips/swarf not being cleared properly
  • Tapping device or machine faulty
  • Incorrect ground or blunt tap
  • Wrong tap selection


EXCESSIVE TAP WEAR 

  • Wrong tap selection
  • Blunt or incorrectly sharpened tap
  • Insufficient or incorrect lubricant
  • Tapping speed too high
  • Hole work hardened

TAPS BREAKING

  • Incorrectly sharpened/blunt tap                               
  • Tap hits bottom of hole
  • Machine or tapping device faulty
  • Wrong tap selection
  • Incorrect or insufficient lubricant
  • Tapping speed too high
  • Hole work hardened
  • Inefficient chip or swarf removal
  • Incorrect tapping drill size

OVERSIZE/BELL MOUTHED

  • Misalignment
  • Incorrect feed rate
  • Incorrect tapping drill
  • Tapping device or machine faulty
  • Insufficient or incorrect lubricant
  • Incorrectly ground or eccentric tap
  • Wrong tap selection

COLD WELDING

  • Wrong material composition
  • Blunt or incorrectly sharpened tap
  • Insufficient or incorrect lubricant
  • Tapping speed too high
  • Material too soft

TAP TEETH CHIPPING

  • Incorrectly sharpened/blunt tap
  • Tap hits bottom of hole
  • Machine or tapping device faulty

In order to minimise problems the following rules should be followed:-

  • Use a pitch controlled tapping attachment
  • Choose the correct lubricant
  • Use the correct type of tap for the job
  • Use the correct tapping drill size
  • Choose the correct speeds and feeds
  • Keep taps sharp. Regrind with a proper machine
  • Ensure accurate alignment
  • Check hardness of material, especially when changing batches
  • Ensure thread gauging is recently certified – they do wear!


TAP TERMINOLOGY


CLASSES OF FIT AND TOLERANCES

The various standards for taps give certain allowances or tolerances for manufacture. Taps are generally manufactured to take advantage of these tolerances, so that as they wear their life is extended. The closest tolerances are applied to Class 1 taps, and the most generous to Class 3. Standard, off the shelf taps are manufactured to Class 2, which applies to all taps listed in this catalogue. Classes 1 and 3 can be manufactured to order.

Classes of fit apply to all thread forms:-

CLASS 1  Produces tapped holes of 4H and 5H fit for Metric threads, 3B fit for American Unified threads and Close fit for Whitworth and BA threads.
CLASS 2 Produces tapped holes of 6H, 4G and 5G for Metric threads, 2B for Unified threads and Medium fit for Whitworth and BA threads.
CLASS 3 Produces tapped holes of 7H, 8H and 6G for Metric threads, 1B for Unified threads and Free fit for Whitworth and BA threads.

Information on tolerances and fits for individual threads is available on request.
 

 

TAPPING DRILL SIZES

METRIC COARSE AND FINE THREADS

THREAD SIZE

DRILL (mm)

THREAD SIZE

DRILL (mm)

THREAD SIZE

DRILL (mm)

M1x0.25

0.75

M9x0.75

8.3

M18x2

16

M1.2x0.25

0.95

M9x1

8

M18x2.5

15.5

M1.4x0.3

1.1

M9x1.25

7.8

M20x1

19

M1.6x0.35

1.25

M10x0.5

9.5

M20x1.5

18.5

M1.8x0.35

1.45

M10x0.75

9.3

M20x2

18

M2x0.4

1.6

M10x1

9

M20x2.5

17.5

M2.2x0.45

1.75

M10x1.25

8.8

M22x1

21

M2.5x0.45

2.05

M10x1.5

8.5

M22x1.5

20.5

M2.6x0.45

2.15

M11x1

10

M22x2

20

M3x0.35

2.65

M11x1.25

9.8

M22x2.5

19.5

M3x0.5

2.5

M11x1.5

9.5

M24x1

23

M3.5x0.35

3.15

M12x0.5

11.5

M24x1.5

22.5

M3.5x0.6

2.9

M12x0.75

11.3

M24x2

22

M4x0.5

3.5

M12x1

11

M24x3

21

M4x0.7

3.3

M12x1.25

10.3

M25x1.5

23.5

M4.5x0.5

4

M12x1.5

10.5

M25x2

23

M4.5x0.75

3.75

M12x1.75

10.3

M27x3

24

M5x0.5

4.5

M13x1

12

M30x3.5

26.5

M5x0.75

4.25

M14x1

13

M33x3.5

29.5

M5x0.8

4.2

M14x1.25

12.8

M36x4

32

M6x0.5

5.5

M14x1.5

12.5

M39x4

35

M6x0.75

5.25

M14x2

12

M42x4.5

37.5

M6x1

5

M15x1

14

M45x4.5

40.5

M7x0.5

6.5

M15x1.5

13.5

M48x5

43

M7x0.75

6.25

M16x1

15

M52x5

47

M7x1

6

M16x1.25

14.8

M56x5.5

50.5

M8x0.5

7.5

M16x1.5

14.5

M60x5.5

54.5

M8x0.75

7.25

M16x2

14

M64x6

58

M8x1

7

M18x1

17

M68x6

62

M8x1.25

6.8

M18x1.5

16.5

M72x6

66

To calculate tapping drill size for metric threads subtract the pitch from the major diameter, Select the next larger standard drill size.

UNC & UNF THREADS

 

BSW

DRILL(mm)

BSF

DRILL(mm)

1/8.40

2.54

3/16.32

3.97

3/16.24

3.7

1/4.26

5.37

1/4.20

5.08

5/16.22

6.8

5/16.18

6.5

3/8.20

8.3

3/8.16

7.9

7/16.18

9.7

7/16.14

9.3

1/2.16

11.1

1/2.12

10.6

9/16.16

12.7

9/16.12

12.2

5/8.14

14.1

5/8.11

13.6

11/16.14

15.6

3/4.10

16.5

3/4.12

16.9

13/16.10

18.1

13/16.12

18.5

7/8.9

19.4

7/8.11

19.9

15/16.9

21

1!10

22.9

1”8

22.2

1.1/8.9

25.8

1.1/8.7

24.9

1.1/4.9

28.9

1.1/4.7

28.1

1.3/8.8

31.8

1.3/8.6

30.7

1.1/2.8

34.9

1.1/2.6

33.9

1.5/8.8

38.1

1.5/8.5

36.2

1.3/4.7

40.8

1.3/4.5

39.4

1.7/8.7

44

1.7/8.4.1/2

42

2”7

47.2

2”4.1/2

45.2

BSW & BSF THREADS

  

UNC

DRILL (mm)

UNF

DRILL (mm)

1.64

1.55

0.80

1.25

2.56

1.8

1.72

1.55

3.48

2.1

2.64

1.85

4.40

2.3

3.56

2.1

5.40

2.6

4.48

2.4

6.32

2.8

5.44

2.7

8.32

3.4

6.40

2.9

10.24

3.9

8.36

3.5

12.24

4.5

10.32

4.1

1/4.20

5.1

12.28

4.6

5/16.18

6.6

1/4.28

5.5

3/8.16

8

5/16.24

6.9

7/16.14

9.4

3/8.24

8.5

1/2.13

10.8

7/16.20

9.9

9/16.12

12.2

1/2.20

11.5

5/8.11

13.6

9/16.18

12.9

3/4.10

16.5

5/8.18

14.5

7/8.9

19.5

3/4.16

17.5

18

22.2

7/8.14

20.5

1.1/8.7

25

1”12

23.2

1.1/4.7

28.2

1.1/8.12

26.5

1.3/8.6

30.8

1.1/4.12

29.5

1.1/2.6

34

1.3/8.12

32.8

1.3/4.5

39.5

1.1/2.12

36

24.1/2

45.3

PIPE THREADS
 

BSP

DRILL

(mm)

BSPT

DRILL

(mm)

NPT

DRILL

(mm)

NPTF

DRILL

(mm)

PG

THREAD

DRILL

(mm)

1/16.28

6.8

1/16.28

6.2

1/16.27

6.3

1/16.27

6.3

7

11.3

1/8.28

8.8

1/8.28

8.2

1/8.27

8.5

1/8.27

8.4

9

13.9

1/4.19

11.8

1/4.19

10.9

1/4.18

11

1/4.18

10.9

11

17.3

3/8.19

15.3

3/8.19

14.4

3/8.18

14.5

3/8.18

14.25

13.5

19

1/2.14

19.1

1/2.14

18

1/2.14

18

1/2.14

17.75

16

21.2

5/8.14

21.1

3/4.14

23

3/4.14

23

3/4.14

23

21

27

3/4.14

24.6

1”11

29

1”11.5

29

1”11.5

29

29

35.5

7/8.14

28.4

1.1/4”11

38

1.1/4”11.5

38

1.1/4”11.5

37.8

1”11

30.9

1.1/2”11

44

1.1/2”11.5

44

1.1/2”11.5

43.8

1.1/8.11

35.6

2”11

55

2”11.5

56

2”11.5

55.8

1.1/4.11

39.6

2.1/2”11

71

1.3/8.11

42

3”11

83

1.1/2.11

45.5

1.3/4.11

51.4

2”11

57.3

2.1/4”11

63.4

2.1/2”11

72.9

2.3/4”11

79.2

3”11

85.6

 
TAPPING DRILLS FOR FLUTELESS TAPS

 

METRIC

DRILL

(mm)

UNC

DRILL

(mm)

UNF

DRILL

(mm)

1.6x0.35

1.45

1.64

1.67

0.80

1.38

2x0.4

1.8

2.56

1.98

1.72

1.69

2.5x0.45

2.3

3.48

2.27

2.64

2

3x0.5

2.8

4.40

2.56

3.56

2.31

3.5x0.6

3.2

5.40

2.89

4.48

2.6

4x0.7

3.7

6.32

3.14

5.44

2.91

4.5x0.75

4.2

8.32

3.8

6.40

3.22

5x0.8

4.6

10.24

4.34

8.36

3.84

6x1

5.6

12.24

5.01

10.32

4.47

8x1.25

7.4

1/4.20

5.77

1/4.28

5.94

10x1.5

9.3

5/16.18

7.3

5/16.24

7.5

12x1.75

11.2

3/8.16

8.8

3/8.24

9

14x2

13.1

7/16.14

10.3

7/16.20

10.5

16x2

15.1

1/2.13

11.8

1/2.20

12.1

BA THREADS

  

THREAD

DRILL

(mm)

0

5

1

4.4

2

3.9

3

3.4

4

2.95

5

2.6

6

2.25

7

2

8

1.75

9

1.5

10

1.35

Calculating tapping drill sizes.

As a rule of thumb, for Metric threads, the tapping drill can be calculated by subtracting the pitch from the diameter of the thread.

e.g for an M5x0.75 thread the tapping drill is 5-0.75mm = 4.25mm.

For Imperial (inch) threads the tapping drill size is calculated in the same way, diameter minus pitch.

e.g for 3/4.10 UNC pitch = 0.1, diameter = 0.75, tapping drill = 0.65 = 16.5mm.