Practical Screw Thread Information & Tolerances

[Gordon Clarke]

Stefanhg;
This statement was true. BS 21 was rescinded and replaced with BS EN 10226 which mimics ISO 7, but there was an outcry from users of BS 21 who did not want to change to the ISO-like gage system, and BS 21 was reinstated.

Now I'm going to have to rethink my last comment (praise) regarding bureaucracy. From what you write Wayne then it appears as if the "new" BS21 was put into motion without surveying with, and/or consulting with the users.
People that sit behind desks in ivory towers shouldn't be allowed to write things that affect real people
I'll bet the bumble bee is glad it can't read or it would be crawling from flower to flower.

 

[Gordon Clarke]

This isn’t the first time this has crossed my mind, but as Whitworth form pipe threads seem to be “in” at the moment I’ll share my thoughts.

A tapered pipe thread is usually used with pack garn or thread tape to seal the joint. If a tapered external thread “R” is used with a tapered internal thread “Rc” then this will give, what should be, a good sealing on several flanks and the bonus of a “solid” joint. On the other hand, if a tapered external thread “R” is used with a parallel internal thread “Rp” then this will only give a sealing on, at best two or three flanks.
I suppose the biggest “dangers” will come from a weakening of the thread’s binding force, a tendency to deform the thread and pipe and last, but not least, a poor leak-proof joint. Why would anyone want to use this combination except in an emergency or when there was no alternative?
Are my thoughts off the mark or is there something I’m missing?

 

[Wayne]

Now I'm going to have to rethink my last comment (praise) regarding bureaucracy. From what you write Wayne then it appears as if the "new" BS21 was put into motion without surveying with, and/or consulting with the users.

That is how I understood the situation too. The British Standards Association instituted the BS EN 10226 and obsoleted the BS-21 under pressure from the EC Standards Committee. Only when they got an earful from the users of BS-21 did they recant and reinstall BS-21.

The primary rub is the design of the ring gages. ISO 7 uses parallel full form ring and then a second plain taper ring to check the tapered external thread. The BS 21 uses a threaded taper ring gage to check the external tapered thread. Otherwise both standards are very much similar. When ISO 7 was in the approval stages both UK and USA objected to the ring gage design.

 

[Wayne]

A tapered pipe thread is usually used with pack garn or thread tape to seal the joint. If a tapered external thread “R” is used with a tapered internal thread “Rc” then this will give, what should be, a good sealing on several flanks and the bonus of a “solid” joint. On the other hand, if a tapered external thread “R” is used with a parallel internal thread “Rp” then this will only give a sealing on, at best two or three flanks.
I suppose the biggest “dangers” will come from a weakening of the thread’s binding force, a tendency to deform the thread and pipe and last, but not least, a poor leak-proof joint. Why would anyone want to use this combination except in an emergency or when there was no alternative?
Are my thoughts off the mark or is there something I’m missing?

I had the same question and when asked I got this answer:

Let us start the explanation using the NPT thread. The NPT thread has loose control of the major and minor diameters. As a result when assembled there is most always two helical leak paths, one along the major diameter and one along the minor diameter. Pipe sealant fixes this problem except in situations where the chemical in the pipe eats the sealant. In this case a mechanical seal is needed and the NPTF thread was designed. The NPTF thread is designed to have a mismatch at the major and minor diameters which deforms under wrench tight condition and thus forms a mechanical seal. As you can figure it takes a good force to deform the entire major and minor diameters along the whole thread. To gain a better seal the male NPSF thread is mated with the female NPTF thread. This combination gets a better seal because of the reduced assembly force required and the concentration of the compressive force at one point which better deforms the threads into each other.

With the Whitworth thread, during the design process I am sure that Mr. Whitworth sought to eliminate the helical leak path by adding the radii. Theoretically this would work, but threads are so full of manufacturing errors that the perfect thread just does not result. Leaks then occur which requires the use of pipe sealant; however; the situation of the chemical being transmitted in the pipe eating the sealant still exists. Now we are back to the use of the male Rp thread with the female R thread to concentrate the pressure at one point and create a mashed together thread and a dry seal.

I believe that is the whole story and full explanation.

 

[Gordon Clarke]

Thanks
That sounds both credible and logical

 

[Gordon Clarke]

Many will already know this, but to those that don’t I find the following very useful and use it often. It is intended for use when manufacturing actual threaded components. If used for a thread gauge, please remember that a thread ring gauge is in fact an external thread inside out and vice versa. I have the same information for Tr and ACME but I’ll wait with those until asked.

FINDING NOMINAL PITCH DIAMETER (d2 / D2)

Nominal pitch diameter (d2 / D2)for a standard thread is often given on the various technical tables issued by companies supplying threaded or thread cutting components. If the major diameter and the pitch diameter for a specific thread type and pitch is known (regardless of the actual thread diameter) then the nominal pitch diameter for the same thread type and pitch can be calculated by simply subtracting PDN from the nominal thread diameter.
A finished external thread should never be above nominal pitch diameter and an internal thread never below.

N.B. Even when the results are given in 0,001mm (0.00005”) or less, it is probably most practical to round the final result op or down to the nearest 0,01mm (0.0005”) . Only when the pitch diameter tolerance is less than 0,1mm (0.005”) should it be relevant to go to 0,005mm (0.0002”) or 0,001mm (0.00005”).
0.001mm is in actual fact 0.00004”.

M (metric) – 60O Pitch in mm
The first number is Pitch (P) in mm, the next is PDN in mm and the inch equivalents for PDN are given in brackets.

P mm PDN mm (PDN inches)
0.5 0.325 (0.012795)
0.6 0.390 (0.015354)
0.7 0.455 (0.017913)

0.8 0.520 (0.020472)
1 0.650 (0.025591)
1.25 0.812 (0.031969)

1.5 0.974 (0.038465)
1.75 1.137 (0.044764)
2 1.299 (0.051142)

2.5 1.624 (0.063937)
3 1.949 (0.076732)
3.5 2.273 (0.089488)

4 2.598 (0.102283)
4.5 2.923 (0.115079)
5 3.248 (0.127874)

5.5 3.572 (0.140630)
6 3.897 (0.153425)
8 5.196 (0.204567)


UN (ISO Inch) - 60O
The first number is Pitch (P) in TPI, the next is PDN in mm and the inch equivalents for PDN are given in brackets.

P TPI PDN mm (PDN inches)
48 0.343 (0.013504)
44 0.376 (0.014803)
40 0.411 (0.016181)

36 0.457 (0.017992)
32 0.516 (0.020315)
28 0.589 (0.023189)

24 0.688 (0.027087)
20 0.825 (0.032480)
18 0.917 (0.036102)

16 1.031 (0.040591)
14 1.179 (0.046417)
13 1.270 (0.050000)

12 1.374 (0.054094)
11 1.499 (0.059016)
10 1.651 (0.065000)

9 1.834 (0.072205)
8 2.062 (0.081181)
7 2.357 (0.092795)
6 2.751 (0.108307)

5 3.299 (0.129882)
4.5 3.665 (0.144291)
4 4.125 (0.162401)


Whitworth - 55O
The first number is Pitch (P) in TPI, the next is PDN in mm and the inch equivalents for PDN are given in brackets.

P TPI PDN mm (PDN inches)
28 0.581 (0.022874)
26 0.626 (0.024646)
22 0.740 (0.029134)
20 0.813 (0.032008)

19 0.856 (0.033701)
18 0.903 (0.035551)
16 1.017 (0.040039)
14 1.162 (0.045748)

12 1.356 (0.053386)
11 1.479 (0.058228)
10 1.626 (0.064016)
9 1.807 (0.071142)

8 2.033 (0.080039)
7 2.323 (0.091457)
6 2.711 (0.106732)
5 3.253 (0.128071)

4.5 3.614 (0.142283)
4 4.066 (0.160079)
3.5 4.647 (0.182953)
3.25 5.004 (0.197008)
3 5.422 (0.213465)

2.875 5.657 (0.227166)
2.75 5.914 (0.232835)
2.625 6.196 (0.243937)
2.5 6.506 (0.256142)


Examples (given in mm) :


M16x2


Nominal major diameter (D/d) = 16,000 mm

Nominal pitch diameter (D2/d2) = 14,701 mm (ref. ISO 724)

i.e. the difference between the major diameter (D/d) and the pitch diameter (D2/d2) is 16,000 – 14,701
= 1,299 mm

Nominal pitch diameter (D2/d2) for a metric thread (M) regardless of major diameter size (D/d) and with a
2 mm pitch, can be found by simply subtracting 1,299 from the nominal major diameter (D/d).


Nominal pitch diameter (D2/d2) for the following metric threads with a 2 mm pitch are :

M16x2 = 16,000 – 1,299 = 14,701
M36x2 = 36,000 – 1,299 = 34,701
M60x2 = 60,000 – 1,299 = 58,701
M120x2 = 120,000 – 1,299 = 118,701


UNC ¼ – 20 (the pitch in mm for 20 T.P.I. = 25,4 : 20 = 1,270 mm)

Nominal major diameter (D/d) = ¼” = 0,250” = 0,250 x 25,4 = 6,35 mm

Nominal pitch diameter (D2/d2) = 5,5245 mm (ref. ISO 725)

i.e. the difference between the major diameter (D/d) and the pitch diameter (D2/d2) is 6,35 – 5,5245
= 0,8255 mm

Nominal pitch diameter (D2/d2) for a ISO Inch thread (UNC, UNF, UNEF, UN etc.) for any major diameter (D/d) and a 20 T.P.I. pitch, can be calculated by simply subtracting 0.8255 mm from the nominal major (D/d).

Nominal pitch diameter (D2/d2) for the following ISO Inch threads with a 20 T.P.I. pitch are :

¼ UNC – 20 = 6,35 – 0,8255 = 5,5245
½ UNF – 20 = 12,70 – 0,8255 = 11,8745
¾ UNEF – 20 = 19,05 – 0,8255 = 18,2245
1½ UN – 20 = 38,10 – 0,8255 = 37,2745

The number to be subtracted fron the nominal major diameter (D / d) to find nominal pitch diameter is hereafter called PDN . The following tables on page 2 of 2 show PDN for a number of standard thread types.

N.B.
Tolerance limits for D2 on a nut are always from nominal D2 and over and tolerance limits for d2 on a bolt are always from nominal d2 and below. This means that the size of D2 for a nut must always be larger than the nominal pitch diameter and the size for d2 must always be smaller than the nominal pitch diameter.

 

[Gordon Clarke]

Can anyone find any holes in my argument for thread measurement contra thread gauge use when setting up a machine and for process control?

0.006 inches is not an unusual thread pitch diameter tolerance and is in fact often more with threads cut using carbide thread inserts. A normal CNC machine should have no problem manufacturing consistently to a diameter tolerance of 0.002 inches or less.

When setting up a machine to run a large series of threaded components it is not unusual that a thread plug or ring gauge is used to “make sure” the thread is OK. The problem with this approach is that the operator “guesses” where the pitch diameter actually is in relationship to the tolerance. If the thread is measured and placed as close as possible to the average pitch diameter as possible then process inspection can be focussed on carbide insert wear or breakage as the pitch diameter tolerance will almost certainly be kept within tolerance.

A GO thread plug or ring gauge should be sufficient at predetermined intervals to check for aforementioned insert wear or breakage. By using the thread gauge when the thread will probably be well within pitch diameter tolerance will mean that gauge wear will be drastically reduced and costly gauge calibration can be given greater intervals.

Apart from pitch diameter measurement (which normally has the smallest tolerance of the three diameter tolerances), a digital caliper can be used to measure the outside diameter on an external thread and for measuring the hole diameter on an internal thread. This method is probably the closest anyone can come to, to achieving “free quality”.

Anyone inspecting a batch of threaded components will know that a much smaller sample size is required when measuring, than if thread gauges are used. Simple calculations can be performed, as threads cut on a CNC machine will probable have a normal distribution. A gauge only reveals too big, too small or OK.

Why do so many companies (especially sub-suppliers), regard thread measurement as complicated? Compared to thread measurement setting up a CNC machine should require a PhD at least!

If threads cut with a tap or a die are measured on the pitch diameter then it will also inform the operator where the thread is in relation to the tolerance. Never forget that standard taps and dies are made to cut standard thread tolerances.

OK, what are the pros and cons of the above statement(s)?

 

[Gordon Clarke]

Screw threads and surface treatment:

Unless you just happen to be in a company that is impervious to the global recession, and never have thread problems then perhaps this could be of interest.

When a cylinder or hole is surface treated (zink, chrome, electro polishing etc.) the amount added or removed is twice that of the actual layer thickness. With a thread the amount added is closer to four times this value as it is applied to all “four” flanks. This often results in that the final component has too "tight" a thread.

A relatively easy and inexpensive way to eliminate this problem is:
1) Determine (measure) what is a normal surface treatment thickness and how much it can vary
2) Specify the thread pitch diameter tolerance before surface treatment
3) Specify the thread pitch diameter tolerance after surface treatment

These three steps are important (critical) because:
Ad 1) It is asking for trouble (or receiving expensive and/or not thought out offers) to not know what is possible and/or problematic
Ad 2) Often standard taps and dies cannot be used and by specifying the tolerance the producer will know what is required and order them special made. If the thread is machined using a carbide thread insert then the specified tolerance can be met without problems.
Ad 3) If attention has been focussed on 1 and 2 then a “standard” thread gauge can almost certainly be used to inspect the finished product. Thread pitch diameter measurement will also show where the pitch diameter is in relation to the specified tolerance.
If the finished product has a problem with the thread then, if the surface treatment process has added material (as opposed to removing material with electro polishing), simply remove the surface treatment layer to determine the actual machined pitch diameter tolerance to see if the machining or surface treating process has been controlled.

If this action seems lengthy or involving “extra” work, remember that a little extra initial effort will quickly become time and money well spent. No problems, no delay, no extra cost and no customer complaints!

If anyone should require more detailed explanations or suggestions to this or my previous “contribution”, then a PM (Private Message) may be necessary. If a question or issue is raised in here then it will also be replied to in here (The Cove).

There are many more methods to measure an external thread than an internal thread, but measuring an internal thread need neither be complicated or expensive. On UN and metric threads the pitch diameter tolerance is usually about 30% greater for an internal thread than the matching/corresponding external thread.

 

[Wayne]

Basically your statements are accurate. Let me add some points for clarification:

... a digital caliper can be used to measure the outside diameter on an external thread and for measuring the hole diameter on an internal thread....

The standard GO/NOGO threaded working plug gage does not measure the minor diameter and a GO/NOGO threaded ring gage does not measure the major diameter. See this webpage for more details. These diameters require measurement via an alternate method from a GO/NOGO screw thread gage. Calipers, micrometers, GO/NOGO pin or ring gages all will work sufficiently.

... inspection can be focused on carbide insert wear or breakage as the pitch diameter tolerance will almost certainly be kept within tolerance. A GO thread plug or ring gauge should be sufficient at predetermined intervals ...

The GO screw thread gage member (ring or plug) does check the maximum material condition. Thus, if wear or damage occurs to the cutting tool, the GO screw thread gage member can be used to detect this change. See this webpage for more details.

I had discussions with a major US bolt manufacturer. They used a modified form of what you propose. They set their machines up using GO/NOGO ring gages and then set-up an external tri-roll gage with functional/multi-rib rolls to monitor the production. Checking the screw thread with the tri-roll was 10-times faster than checking with ring gages. This almost eliminated wear on the ring gages, and as we know, tri-rolls do not wear quickly either.

 

[Gordon Clarke]

Basically your statements are accurate. Let me add some points for clarification:.

Wayne, thanks for a very useful response and I'm in the process of writing a reply. My immediate reaction to what you wrote was a paranoid "I'm being critized :mg:", until I realised that it wasn't the case

We have the same ultimate goal - just slightly different approaches - slightly being the operative word