Help selecting insert for whitworth threads

I need to cut some 16tpi, Whitworth threads in 4140 steel. I'm planning to use an NSR08-2J toolholder and would like to find the appropriate insert. I've been up to CarbideDepot and looked over the million or so options from MSC, but would like to buy with confidence that I have the right one. Can someone please point me in the right direction. Also, if you have another approach, feel free to share it. I have five of these to do and am just looking for the right tool for the job.

Thanks!
Joe

Another approach:
Iscar, maybe you never heard of it before.
www.iscarmetals.com

Whitworths have rounded profiles. You can't just run a file over the top and
say you are done.

Another point is that the Whitworth thread form has a 55 degree included flank angle. Good luck. If Whitworth threading inserts are unavailable, find a GP unified thread insert and have a tool shop regrind it to 55 degrees and doctor the tip radius.

Don't be tempted to use a 60 degree thread insert unmodified. In high confidence fasteners the flank angles have to match pretty closely. 2 1/2 degrees flank error on a side is asking for a gall when torquing. The wrench might click but a gall could trigger it aqnd leave the fastener way under-tensioned.

In practice most modern Whitworth threads are truncated flat rather than rounded. Can't lay my hands on the spec right now tho' but it is officially permitted. Basically its H/6 plus depth of rounding where H is thread depth, 55 degree remember, best to look it up. Watch out for tolerances and fit classes if the job needs them as the Whitworth methods predate modern thinking and they have never been properly bought into line. Tolerance and fit classes are much more important if you do round the ends. Things can jam and gall quite spectacularly if you get it wrong. Especially in stainless. Whitworth form is the basis for quite a few special, often precision, applications which tend not to follow normal nut & bolt standards.

As Forrest says 55 degree and 60 degree flank angles don't mix.

Best approach is to treat the job as a special and do it as the books say for that size and application rather than try to work out from standards.

Found the truncation data, its in Machinery's Screw Thread Handbook and is the depth of rounding. Supposed to compensate by adjusting the thread shortening but that's hardly worth it unless the TPI is small. For your 16 TPI the truncation is 4.62 thou and the thread depth is 40 thou (for all practical purposes). Hence if you start by over-cutting the bore or male component by the truncation depth you get near as dammit 75 % engagement. Good enuf for engineers nail jobs. half the truncation depth for a closer fit.

Clive

Joe,

Carmex makes a full line of Whitworth inserts. Partial profile and full profile.

Ray

Hello Ray,

Are they available here, or just listed in the catalog?

My experience is that there are many manufacturers that list them in the catalogs, but good luck finding them in the US, other than 55° inserts for BSP!


Fractal,

Some of the stuff I work with is close tolerance BSF threads, so I have resorted to grinding my own HSS tool bits (manual lathe) using a Compound Magna-Sine on the surface grinder and stoning the tip radius by matching the profile to a similar close tolerance threaded part until the tool bit fit is "light tight" in the groove. As previouly mentioned, on my stuff, trincation of the crest is permitted on close tolerance BSF threads.

Just an option!

Still searching for those Whitworth Thread Wires though! Using a conversion to UN wires now.

Glenn,

Yes, Carmex has most sizes of Whitworth in stock. MSC can order from them if they themselves don't stock, or you can order direct from Carmex. Their number is: 888 628 5030. Helpful people!

Ray

Thank You Ray!

Kennysmetal has some in Top Notch and other in Lay Down.


---------

Think Snow Eh!
Ox

Thanks!

All,
Thanks for your input. I'm aware of the 55* profile as well as the radii at the root and crest of the thread which is why I'm trying to find an insert rather than attempting to grind my own. I'll give the ISCAR a look but it seems like the CARMEX is the best bet for a starting point. Again, thanks!
Joe

Ray Behner said:

Joe,

Carmex makes a full line of Whitworth inserts. Partial profile and full profile.

Ray

Click to expand...

Ray,
With partial profile inserts, how do you produce the rounded over crests which
a full profile insert would produce?

Ron

rons said:

Ray,
With partial profile inserts, how do you produce the rounded over crests which
a full profile insert would produce?

Ron

Click to expand...

Ron,

I don't even know why they make partial profile. I never use them. I guess pp's are ok for some stuff but I like cresting the thread. Looks better, works better. I was just saying what was available.

Ray

Thanks Ray.

Ron and Ray,

Bottom of Page. (American Machinists Handbook)

Glenn.
Whenever somebody posts a drawing or picture that means some effort.
Thanks. The truncated thread was what the original question was about.

You might look at Brownells, Mausers are also 55 deg.

Have purchases 55* lay down inserts from Sandvik...was not a problem getting them as i recall...had the inserts the next day after the phone call.
Cheers Ross

Glenn, Rons

Nice table but unfortunately the truncation figures given don't appear to agree with those given in my 18th edition (1961) of Machinery's Screw Thread Handbook. However the figures given refer to maximum deviation from nominal not the actual truncation so will include fit allowances and tolerances whilst the Machinery's book basically defines truncation and tell you how to calculate the rest.
Fit allowances and tolerances are a bear to calculate with Whitworth form at the best of times. Even the standard formula uses the square root of pitch twice as well as a fraction of a horrible factor e one of whose terms is the cube root of the major diameter. Just to make matters worse a lot of Whitworth stuff will be to Newall System tolerances (i.e. bilateral) rather than modern ISA / ISO (unilateral) so you may have to figure out what the appropriate major diameter is to start with if you are doing precision work. Most of the special applications have their own over-riding tolerance limits too. Fortunately usually stated in (relatively!) simple terms.

The truncated thread form is a bit simpler as at least the basic tolerances for major diameter of the screws and minor diameter of nut are pretty straightforward being 0.052165p + 0.003" on bolt major diameter and 0.052165P + 0.004" over 26 tpi, + 0.004" for 24 and 22 tpi, and + 0.007" under 20 tpi where p is the pitch.

These days if you really needed to calculate things its not too difficult to set-up a spreadsheet but in slide rule and mechanical calculator days it must have been a nightmare. I wonder how much stuff was actually made to official tolerances rather than the practical near enuf.

Out in the real world truncation makes no practical difference to thread engagement (leaving aside horrible things like the Wreathall mount standard for IR lenses and telescopes) so there is no great point in worrying about rounding unless there are serious stress problems. Frankly its a lot easier to simply say that thread height is 0.96p, thread depth is 0.64p, truncation is 0.075p where p is pitch and pick the appropriate tolerances and fit allowance dimensions off ISO / ISA tables for the equivalent 60° thread.

BA may be a pain to cut but at least the tolerances are straightforward.

Clive

My handbook is a 7th edition, around 1937.

Fortunately, the prints I work from have specifics on them so I don't need to do any calculations.

Example:

.673" to .677" dia before threading
.6875-14 BSF Thread
PD .6426 to .6402

The parts are 1940's and dead on the print dimensions.

"Mausers are also 55 deg"

Yep, and I'll bet there's a million of them that have been rebarreled with 60° threads.