Single point Whitworth Threads

[Jon GibbsParticipant @jongibbs59756]

I hope someone can put me out of my misery please.

I have been trying to cut spindle nose threads to match my ML7 which is obviously Whitworth form but I don't have the right form tool to round the creast and roots. What is the best way to single-point thread these – particularly with a simple 55 degree point tool?

Looking at the trig, starting with the nominal diameter the thread depth of 0.64 x p isn't deep enough to cut the correct flanks. It looks as if it should be 0.82 x p and that leaves a flat crest which still won't mate with the female thread roots..

Is this truncated form the way to go? Apparently it was the way the US machinists made parts to fit UK standards in WWII?

If so any guidance as to the outside diameter – obviously less than nominal but by how much? It's obviously slightly bigger than (nom – 0.36 x p) but I'm struggling with the intersection of the flank with the radius'd top.

Any guidance gratefully received – Many thanks

Jon

[Jon GibbsParticipant @jongibbs59756]

[Ady1Participant @ady1]

If you can move your tool along a tad before the required depth is reached then you can widen the root

so you cut on a single flank to widen the root area

i.e. the line which intersects the c in "pitch". Move the tool along so the line intersect/cuts at t

(only a suggestion)

The usual route I presume would be to finish with a thread chaser

Edited By Ady1 on 23/05/2014 09:21:56

[Les Jones 1Participant @lesjones1]

Hi Jon,
I have found out that the crest and root radius is 0.13733 x the pitch. As I do not know the pitch of your thread I cannot do the calculation. Here is the link to where I found this information.

Les.

[Bob Brown 1Participant @bobbrown1]

When cutting threads I normally off set the compound slide to just over the thread angle so that the tool is cutting most of the material on one flank and only a minimal cut on the other flank, takes a bit of trig to calculate depth but easy enough to do.

The OD is in this case 1.125" the only reason to truncate the thread form is speed of production, after all there was a war on.

The root is normally taken care of by the tool by just add a radius to the tool tip, crest can be taken care of with a chaser or just carefully rounded off with a file.

Or you could either rough it out on the lathe and then run a die down it to clean up the root and crest, RDG sell both taps and dies.

If you were going to truncate then it should only be about 0.017" off the diameter for this thread

 

Bob

Edited By Bob Brown 1 on 23/05/2014 09:55:36

Edited By Bob Brown 1 on 23/05/2014 10:06:24

[Michael GilliganParticipant @michaelgilligan61133]

Jon [and Les]

Here is a better image of the one that Les found.

Although the Decimal calculation looks tricky, it's worth remembering that Whitworth designed the profile by simplly truncating the crest by H/6 and then blending it as a smooth radius.

Use the same process when grinding your tool and " job's a Good 'un "

MichaelG.

Edited By Michael Gilligan on 23/05/2014 10:17:32

[Jon GibbsParticipant @jongibbs59756]

Thanks for all of the replies and suggestions.

I should empahsised that I have made a spindle nose that works ok but I'm just not convinced that the thread flanks are meshing properly as I ended up with well defined crests. So I suppose was looking for a better way.

I think I might have found something here though…

**LINK**

in "Appendix A: Truncated Whitworth form threads with flat crests" gives the flat topped form.

[Incidentally it's quite amusing to see a Chinese company providing a pdf of a British Standard (84:1956) which is labelled as being licensed to South Bank University. BSI will helpfully provide me the same pdf for £204.]

…I'm not sure whether my pedantry in trying to get this better is typical of Myford bods or Flat-earthers

but either way I think I can cope.

Jon

[Michael GilliganParticipant @michaelgilligan61133]

That's a great find, Jon

Thanks

MichaelG.

.

P.S.  it's worth going back to the parent page and browsing

… amongst all the Chinese characters, there are some familiar numbers.

Edited By Michael Gilligan on 23/05/2014 12:10:14

[Gordon WParticipant @gordonw]

I would be more worried about the sharp angle at the bottom of the thread. Stress raiser. Non myford flat earther.

[Ady1Participant @ady1]

I'm only a metal bodger but spindle threads are quite important because they do important stuff, so it's worth getting them right if you can

gl

[Jon GibbsParticipant @jongibbs59756]

Hi Ady,

I agree but I'm sort of assuming that the flanks are more important that the crests or roots which is why I'm trying to take the Myford-bod/flat-earther stance here .

I suppose I also was under the impression that it's the spindle register that provides the concentricity – is that right?

Jon

[Neil WyattModerator @neilwyatt]

If you want the perfect thread form Tracy Tools have three new set of chasers available, using coventry die heads with a holder at £25 a set. I've tried one and it works. You could use it for cutting or finishing these threads. More information in the next MEW or click HERE

Neil

[Jon GibbsParticipant @jongibbs59756]

Ok, so checking through my Trig again, the idea of making the major diameter smaller by 0.1478p before single point threading then the crests will be spot-on without needing rounding. This is the same as taking off the U value in Table 21 of BS 84:1956.

For the Myford 1 1/8" x 12TPI this means the diameter will be 1.113" instead of 1.125".

This means the thread depth with a perfect 55 degree point would need to be 0.9605p (full height) – 0.16p (height / 6) – 0.0739p = 0.7266p. Anything less than a perfect point will need less depth so I guess cutting until thread fits should mean the flanks are meshing ok.

Does this make sense?

Jon

 

Edited By Jon Gibbs on 23/05/2014 14:49:57

Edited By Jon Gibbs on 23/05/2014 14:52:47

[Jon GibbsParticipant @jongibbs59756]

Thanks for the suggestion Neil.

I will give it some thought and see whether my pocket money will stretch to one.

The problem I see with that approach is that It's only good for external chasing isn't it?

Jon

[Jon GibbsParticipant @jongibbs59756]

Here are my thoughts if it makes it any clearer…

Jon

[Jon GibbsParticipant @jongibbs59756]

Sorry for thinking on-line but taking Ady's original suggestion though, the depth could be cut to a smidge over 0.5664p and then broadened until the thread fits which would be better from a stress point of view wouldn't it?

…but is there a way to do this easily with the top-slide set over at 27 degrees?

Jon

[Roderick JenkinsParticipant @roderickjenkins93242]

On my S7 the spindle thread diameter is 1.124" which suggests that it is not a true Whitworth thread form, although it is 55 degrees. The crests are fairly sharp. I think Myford relied on the register to locate the chuck so the backplate threads can be cut fairly loosely with a pointed tool.

cheers

Rod

[Ady1Participant @ady1]

…but is there a way to do this easily with the top-slide set over at 27 degrees?

I would mark the gearwheels off in the geartrain at the start point

Once I reached "not quite deep enough" I would then disconnect the geartrain and advance one gear by a couple of teeth, advancing the leadscrew start slightly but not moving the tool

this would advance your tool into one side of the flank without going any deeper

Edited By Ady1 on 23/05/2014 16:46:13

[Jon GibbsParticipant @jongibbs59756]

Ady,

…Blimey, That will require me having a few minutes to get my head around in a darkened room!

…but seriously, thanks. I guess I will have to try it and see.

Jon

[Neil WyattModerator @neilwyatt]

Hi John,

My set only goes down (up?) to 14 tpi and I've just tested it, set sideways in the holder, and it would be possible to work it inside a 1 1/4" bore with ease -BUT it would be a left-hand thread….

The other way to cut or finish a 12 tpi internal thread would be to use a 1/2" Whitworth tap.

Neil

[Clive FosterParticipant @clivefoster55965]

Methinks the method given by Ady has far to risk of operator confusion leading to major mess-up.

Best to use what was taught to me as the "Zero to Zero" method for screwcutting using the top-side set over at an angle which will allow you to do such broadening cuts at the base of the thread with minimal risk of getting lost. The major advantage of the Zero to Zero method is that it not only does it avoid all the tedious trigonometry to calculate thread depths and sidesteps any errors due to the top-slide angle being a touch off it also gives you an accurately measured account of what you ahve done so if things don't fit you have a fighting chance of figuring out what the gremlins did this time.

Basic method is to turn or bore the workpiece to the correct size then mount the screw cutting tool and bring it up to just touch the workpiece. Set both to cross and topslide dials to zero. Pull the tool back clear of the workpiece and crank the saddle along until the tool point is in clear air. Using the cross slide move the tool back past zero until the dial reads the depth of thread to be cut. Set the dial back to zero and use the topslide to bing the tool back far enough to make the first cut. Use the cross slide to pull the tool into and out of cut for saddle travers, cutting passes being made with slide on zero. Cuts are put on with the top-slide. Job done when top slide at zero and last spring cut is clear.

Obvoiusly the lathe does all the trigonometry to calculate the top-slide feed needed to achieve the desired depth of thread for whatever angle its set at. Which only needs to be close to half the angle of the thread. My topslide lives at 25° off which works just fine for both 55° and 60° threads.

If you need to widen the base of the thread make a cutting pass with the cross slide set a little short of zero with a compensatory extra in-feed on the top-slide to keep the depth the same. For all practical purposes the extra width at the base of the thread will be half the cross slide shift when a compensatory top-side feed of 1.15 times the shift is applied to keep the depth constant. The trig is relatively simple if you want more accurate values but whether your lathe can deliver them is a whole n'other matter.

Frankly is far easier to truncate the threading tool to the proper width tip, maybe stoning a radius on the corners too for a perfect job, than mess around with threading techniques. I've seen some right difficult ways of measuring tool truncation. The easy way is to grind it sharp, measure the overall length, figure out how much shorter it needs to be to give the right width at the end and trim it back by the required amount. If you are confident in your trig the amount to trim is easily calculated otherwise refer to thread data book which will tell you how much the real thread is truncated by when compared to a sharp triangle.

Clive

[Jon GibbsParticipant @jongibbs59756]

Thanks Clive. I think I could probably do the widening that way although my old ML7 is so crude it only has fixed dials on the cross-feed and topslide.

…but when I think about it though, the 12 TPI roots only require taking just over 13 thou off the point of the 55 degree point tool. So it's probably not too bad even if I have to regrind it again afterwards for other thread sizes.

So the way to go for this "bodge" would seem to be to take off the 0.1478p from the major diameter and then with a rounded off point tool (taken off by 0.1600p) go in 0.5664p or maybe a smidge further until it fits?

I'll give it a try over the w/e

Thanks again

Jon

[BubbleParticipant @bubble]

Hello all

When single-point cutting threads, I find that the crests can be rounded off using one of my thread files.

They are designed to be used manually to clean up bruised threads, but I use them in the lathe with the lathe rotating under power at slowest back gear speed.

The file is applied to the threads and not moved, but with the work located on one of the cross-grooves in the file.

The file then acts just like a chaser. (I am a grown-up so please don't anyone tell me its dangerous. I know it's frowned upon, but many time-served machinists used files in the lathe, they just didn't boast about it. If you are not sure about it don't do it.)

The advantage is that each file has 8 different pitches. I have three files, BSF,Whitworth and BSP so 24 chasers although there is overlapping of pitches, all being 55 degree thread angle.

Works for me.

Jim

[GeorgineerParticipant @georgineer]

Though I am reluctant to exhume a thread which died eight years ago, I feel it's important to correct some incorrect information within it to avoid misleading future readers of this thread

The original diagram comes from the website of the American firm Gage Crib Worldwide and is based on a lot of incorrect assumptions, not least of which is that the truncated Whitworth thread didn't comply with any standards. In fact it was fully specified in B.S. 84-1940 (Amendment No. 3, August 1945).

In particular, the thread root was not a V, but had the same profile as the 'normal' Whitworth thread.

I have emailed Gage Crib to offer them corrected information. It will be interesting to see if they respond.

George

[Chris CrewParticipant @chriscrew66644]

I have made several back-plates for my Myford, both from noggins of mild steel and un-machined cast iron blanks. I have cut the threads on my Colchester. I can't say that, apart from the major and minor diameters of the thread and a slight rounding of the point of the screw-cutting tool that I have paid much attention to the precise details of the thread, except obviously for depth, but I have paid a little more attention to the registers. The back-plates screw on and off the lathe freely and the chucks appear to remain concentric. I always cut internal threads on the rear of the hole with the screw-cutting tool inverted in the tool-post and the top-slide set over to half the included angle. Using this method means you don't have to grind a tool to the precise angle because the rear flank is formed by its advance into the work and you don't have to think about which way to withdraw the tool at the end of the cut as it is withdrawn, as of habit, in the same direction as cutting an external thread, you also have a better view of the thread forming as the tool enters the work.

[Author]

Posts