Threadcutting in the lathe – help please!

[ManofkentParticipant @manofkent]

Hello. I am hoping some of you clever people out there can help me.

I am trying to learn how to cut threads in the lathe. I have an emco CNC lathe to practice on – not with any great success at the moment, and have tried to cut a 3/8" Whitworth thread with a 55 degrees tool, 16 tpi.

The puzzles are as follows:

1. If I measure a bolt of the same size it has a diameter of less than 0.375 – more like 0.360 or thereabouts. Do I start with a bar turned to exact 3/8 or do I start with a smaller bar – and if so how do I know how much smaller?

2. My biggest puzzle is how deep to cut the thread. In my reference book there is a figure h/6 = shortening, where h = angular depth of thread (whatever that is!). It looks like this could be the difference in bar diameter referred to above and ditto at the foot of the thread. So if my bar is exactly 0.375, and h is given as 0.0600, and therefore is h/6 0.01?

Do I cut to thread depth h (0.06) minus h/6 – 0.0100 – i.e 0.05? Or do I use the figure shown for depth of thread 0.0400?

3 Is there someone who can explain the difference between core diameter (0.2950) and Effective diameter 0.3350 please.

My book is "Machinery's screw thread book published in 1943!!

My apologies for these questions – I expect it is all blooming obvious – but not to me yet.!

Thanks in advance.

John

[ManofkentParticipant @manofkent]

[Mick B1Participant @mickb1]

You aren't the only one befuddled by mysticism here. I've been cutting threads for over 40 years and still can't answer your questions truly definitively, BUT:

1. I'd start from nominal diameter less a couple of thou – like a bit of 3/8" BDMS round bar would typically be – then

2. Cut the thread by successive passes of decreasing depth as I came close to nominal thread depth, trying a test nut on it each pass for the last 5 thou or so.

3. Effective diameter is the diameter to halfway up the thread flanks. It seems to me to be an artificially theoretical dimension – fiendishly difficult to measure with anything normally available and only of significance in instrument work of the highest precision.You could purchase prepared coils supplied with dimensional tolerance tables to enable you to measure it by the 3-wire method, and in the Government Training Centre where I learned they actually ran through the calculations – but it was clear enough they never expected anybody to actually have to use it, and I never have…

[Jon GibbsParticipant @jongibbs59756]

Hi John,

I'll do my best but IME you have picked the hardest thread-form to replicate first

[Edit: Legend added: A diagram of an ISO metric or Unified thread, showing dimensions relative to the pitch (P) and thread height (H). Note that while diferent standards, ISO and UTS share the same geometry, but not absolute dimensions. Also shown is the location rounding permissible in internal (dark grey, top) and external (light grey, bottom) threads. Key P: Pitch H: Thread height Dmaj: Major diameter Dmin: Minor diameter Dp: Effective pitch diameter Do not scale from this drawing.]

The best economical way to compare threads is using measuring wires (Available from Arc Euro Trade) and a micrometer. With wires you are effectively measuring part way down the flanks of the thread and so you can tell if the profiles are the same between a reference and your attempt – or indeed when using conversion tables you compare to the given effective diameter which is the diameter half way down the flanks. See the picture.

Whitworth has a rounded crest and root which can be difficult without a chaser or a die of some form. So, it is not uncommon to truncate the crests (at a smaller nominal diameter) effectively to a flat as would be the case in the metric and US 60 degree threads.

If I could recommend a new book to you. Try Martin Cleeve's "Screwcutting in the lathe". It's cheap but very good on all things related to threadcutting.

I hope this helps. Happy screwcutting! 

Jon

Edited By Jon Gibbs on 20/06/2018 08:59:19

[JohnFParticipant @johnf59703]

Hi John, cannot help with CNC but as far as the thread is concerned here goes — the H6 probably refers to the thread stand of H6 which is a tolerance for general thread specification.

Regarding cutting the thread and dimensions: the OD is 0.375 the fact that you have measured commercial bolts etc and find them undersize is not surprising but the actual diameter is .375 however if you are not using a full form single point tool [usually a disposable tip type tool] then you will not be cutting a crest radius so it is necessary to truncate the thread i.e. reduce the OD by a few thou, as guide if you use half the crest/root radius you will not be far out in this case the rad is .0086" so make the OD 0.371"

Set your tool to the OD and use a depth of 0.038" —- nominal 0.040" less half the truncation this will give you a very close fitting thread and you may need to gauge this and go an extra 1 or 2 thou to make an easier fit — depends on what you are using the item for. For most ME work as long as it fit your other component it will be just fine, if you want to be sure use either a correctly made thread ring or calliper gauge or a thread micrometer but most people will not have any of these. An alternative is to use the 3 wire method and standard micrometer to measure the effective diameter — a gauge point on the thread flank.

If you want more info on the gauge point etc let me know and I have some tables etc I can send to you – cannot post due to copyright I guess.

John PS where are you located ? nothing in your profile ?

[Mick B1Participant @mickb1]

I see I was lying about Eff Dia being halfway up the thread flanks – it's where the width of the thread profile is half the pitch.

I looks as if your h/6 dimension can be confused with an H6 fit tolerance range – which probably hadn't been defined in 1943.

[HopperParticipant @hopper]

Don't get too bogged down with threadform minutiae and measuring methods. Most professional machinists never refer to the threadform diagrams and get by using traditional rules of thumb.

First is to always make the OD a few thou smaller than the nominal. So make your 3/8 BSW from a bar that is turned to.365 – .370" diameter. If you don't, the finished thread will bind on the tips of the threads. There needs to be clearance there. Commercial threads, as you have seen, are mass produced at even smaller diameters, to ensure all nuts screw on to all bolts. You can go down to 85 per cent thread engagement and not lose any significant strength. Even 65 per cent engagement is over 90 per cent of full strength. (See Tubal Cain's ME Handbook.) So do not sweat the OD as long as it is smaller than the nominal by a bit.

Second is for 55 degree thread form (BSW etc) make the nominal thread depth .6403 x Pitch. Your pitch for 16 tpi is 1 divided by 16 = .062". So thread depth is .6403 x .062" = .0396", call it the .040" in the previous post.

Third is don't sweat the root and crest radiuses. Rub the tip of the tool on an oilstone to round it off a bit and call it good. Then use a file to round off the tops of the threads as you remove the inevitable burrs and call that good. The roots and crests are clearance areas so there is no need to sweat making exact radiuses, or flats or whatever.

Fourth is to get final depth of cut and finished thread size by "sneaking up on it" in small cuts and checking the fit of a nut or the mating threaded component as you go. So don't sweat the exact depth of cut. Do it by feel when screwing on the test female thread.

Fifth is to save yourself a lot of aggro and time and use a die or die nut to get the final finish on the thread, just that last few thou. If you have a die or die nut. If not, don't sweat it and follow the above procedure.

+1 on recommending Martin Cleeve's book Screwcutting in the Lathe. Also LH Sparey's The Amateur's Lathe.

Edited By Hopper on 20/06/2018 09:49:09

Edited By Hopper on 20/06/2018 09:56:04

[Jon GibbsParticipant @jongibbs59756]

Posted by Mick B1 on 20/06/2018 09:28:47:

I see I was lying about Eff Dia being halfway up the thread flanks – it's where the width of the thread profile is half the pitch.

I think you were right – if you extend the thread flanks from one peak to the base of a perfect trough it is half-way i.e. H/2 down or up.

Jon

[Ian S CParticipant @iansc]

When I was at school we were shown how to cut Whitworth threads, when the thread will almost fit a nut, the thread tool was replace by a hand held thread chaser to cut the top and bottom radius. I,

I'v just come across a box full of inside and outside chasers, they need handles.150 yrs ago and threads were cut free hand with a chaser on a foot powered lathe.

Ian S C

Edited By Ian S C on 20/06/2018 10:24:26

[LambtonParticipant @lambton]

John,

I fully agree with all that Hopper has said.

My late father, a skilled RAF trained toolmaker, taught me to finish off a single point screw cut thread with a die or die nut. You can also use a thread repair file to chase along the thread. I always give a vigorous wire brushing over the finished cut thread to remove any burs and debris.

The radius at the root of the thread is there to prevent a sharp root from being a stress raiser thus weakening the thread. However do not bother with the crest radius as it serves no practical purpose.

Just use the data in Zeus chart book as this contains all you need to know.

Eric.

[ManofkentParticipant @manofkent]

My thanks to everyone. Excellent advice from all of you.

I think I was probably looking for problems – when like most things it is a matter of experience (thanks Hopper).

The book is on order!

I turned the stock to 0.372"

So I wrote the program and with buttocks appropriately clenched cut to 0.04 depth at 0.001" per pass. easy to program on CNC but you have limited options to check it half way through!.

(For any Emco CNC users I used program G78 to cut the thread).

Still it seemed to work OK, except the thread was pretty "raw" on its edge, I had to be careful not to cut my hand on it!. A quick run over with a die and it was pretty perfect really.

really grateful for your help.

John

[JonParticipant @jon]

Very good Jon and Hopper.

Presume some advice is using a ground up tool V tool creating no root, with full form tips you could have the diameter well oversize and end up to desired tolerance if any for max strength.
Careful with aluminium and titaniums they bind even undersize with no warning, more you twist the more it locks up tererible stuff.

John roughness could be a number of things from tool to material and speeds. One thing almost guaranteed to work is within last 0.08mm take minimal cuts off and end up on size sending down again.
Coolant may make it better or worse, suck it and see.

[Mick B1Participant @mickb1]

Other question re: finish in my mind is –

Does the program simply plunge the tool in by 0.001" per pass; or does it offset it, so as to do the CNC equivalent of half-angle screwcutting on a centre lathe compound slide?

Taking material with one side of the tool only eases the cut and usually improves resulting finish.

[Pete RimmerParticipant @peterimmer30576]

One thing that catches many novices out is that often threading a piece of stock will raise a burr which makes you think that the thread's not deep enough when in fact it's binding on the major diameter when you try the nut. You start to wonder if you've got your sums right because you've hit the full depth and the nut is nowhere near fitting so you keep taking cuts until the nut fits but then you find it's a sloppy fit and you don't know why.

Use a caliper to keep an eye on the OD after you have taken a few passes. If it's started to grow because you've pulled up a burr just carefully run over it with a flat file taking long smooth strokes as the part is turning. On a vee thread it won't take many strokes but on an acme/trapezoidal thread you might have to go at it several times to file the burr down to the correct OD.

[ManofkentParticipant @manofkent]

Mick: I am afraid with the cnc machine it is a plunge in approach. Even a cut at 0.001" seemed quite big towards the end.

Jon – The machine was running at about 200 rpm – I did use coolant, but I did not take a couple of cuts at the end as you suggest (and as I remember now seeing others do).

I have identified some full form tips for 60 degree threads which came with the machine. These do look really useful. Presumably though a different size tip is needed depending on the pitch?

BTW thanks to John Gibbs for posting the thread diagram earlier. I get now why Whitworth threads are harder.

I remember a box full of thread chasers in the back of a cupboard somewhere. Next week I will see if I can lay my hands on them.

Thanks John

[HopperParticipant @hopper]

Great that you got a result! Yes, the full form tools with the crest profile ground into them will skim that burr off the top, and would presumeably be what standard CNC programs are designed to work with. But yes you do need one tool for each pitch then, which is not too bad for metric but gets complex for BSW and UNF etc. If using the 60 degree ones to make UN or Metric threads, note the slightly different formula to arrive at thread depth: Depth = Pitch x .6134.

In general practice, Whitworth form is no harder to deal with than the others. As said earlier, the root and crest radius/flats is not critical as these are clearance areas. I usually just run the corner of a flat file down the thread as it revolves to knock that burr off and round the crests at the same time. (Unless you are doing super-precision work for aerospace etc that must pass rigid inspection and the like. But for home hobby work, keep it simple.)

Sometimes neat cutting oil, or even straight machine oil, squirted on the screwcutting job works better than coolant.

If you are grinding your own HSS tools, keep them razor sharp with an oilstone to minimize that burr, and grind them with a bit of extra clearance angle on the leading face, so you have the normal clearance angle plus the helix angle of the thread. Otherwise the face will rub and not cut well at all, leave burrs etc. Honing a radius on the point of the tool with the oilstone also makes it stronger and less likely to break off, which also cuts poorly then.

[ManofkentParticipant @manofkent]

Pete – thanks for your comment. I think this may be why my previous attempts (on my ML10 lathe) seemed to end in the scrap bin. Now I know what to look out for.

Hopper – I can just about grind a HSS knife tool. Getting a Whit profile to the right angle and depth might be pushing my luck. However, you never know till you try, so would there be a profile or type of grinding wheel you would suggest to use given the small size of the tool?

Many thanks

Johm

[HopperParticipant @hopper]

So, what tool are you using for your current Whit. thread turning? It may need sharpening to help reduce burrs. Diamond lap or file will touch up carbide tools.

For HSS you can just use a common-a-garden six inch bench grinder. What size toolbit blank does your lathe take? If it is say, 1/4" square, you just grind a 60-deg point on the end, full width, with suitable clearance on each face. Then smooth it off on a bench oilstone and stone a radius on the very point of the tool. You use a screwcutting gauge to make sure you have the angle right — it's basically a piece of thin steel sheet with a series of 55 and 60 degree notches cut in it and you grind the tool to fit, holding it up to the daylight to look for gaps etc.

[ManofkentParticipant @manofkent]

Hi Hopper

For this exercise I was using a HSS ground tool like this one: https://www.chronos.ltd.uk/cgi-bin/sh000001.pl?WD=threading%20hss&PN=HSS_DOUBLE_ENDED_THREADING_TOOLS%2ehtml#a136220.

It feels like a bit of a blunt instrument really, and probably does need sharpening now.

If I have a lot of threading I think something like this would be needed: https://www.cutwel.co.uk/thread-making/indexable-threading-single-point-threading/whitworth-threading-inserts/external-right-hand-whitworth-threading-inserts

I was actually thinking I could make my boiler fittings on the lathe – ME threads 40 and 32. It is all a learning opportunity and I love learning new skills.

JohnF – I updated my profile but essentially I am in Taunton and a member of the excellent Tiverton Model Engineers club.

John

[HopperParticipant @hopper]

Looks like it should do ok. Bit of a touch up on the oilstone might help.

For small threads like model boiler fittings, most people will use a die in a tailstock holder. Works better and easier on that small stuff, short length, brass material. But you could screwcut it. Brass screwcuts quite nicely with HSS tools.

[Mick B1Participant @mickb1]

Posted by Hopper on 21/06/2018 07:48:12:

…

For HSS you can just use a common-a-garden six inch bench grinder. What size toolbit blank does your lathe take? If it is say, 1/4" square, you just grind a 60-deg point on the end, full width, with suitable clearance on each face. Then smooth it off on a bench oilstone and stone a radius on the very point of the tool. You use a screwcutting gauge to make sure you have the angle right — it's basically a piece of thin steel sheet with a series of 55 and 60 degree notches cut in it and you grind the tool to fit, holding it up to the daylight to look for gaps etc.

That's more or less what I've done since 1975. At 16 TPI, a cheap pitch gauge its probably good enough to get the angle with sufficient accuracy. I still use a similar tool I ground that way when I was starting out – all I've done is touch up the top and tip a few times since – though it's true I only tend to use singlepoint screwcutting when no easier method is available or adequate.

[SillyOldDufferModerator @sillyoldduffer]

Posted by John Hilton on 20/06/2018 08:21:11:

 

 

…

My apologies for these questions – I expect it is all blooming obvious – but not to me yet.!

Thanks in advance.

John

Not obvious at all, including the possibility that you're making life difficult by working to an unnecessarily tight specification, and have started with a 'difficult' thread.

Whitworth threads are glorious because they swept away anarchy. Before Whitworth every Tom, Dick and Harry made their own threads, and of course they were all incompatible. Whitworth was a good thread for general engineering work and is particularly well suited materials common in the 19th century like cast iron. It's not a good choice for light engineering, clocks, and electrical applications, nor is it ideal for modern materials.

One early criticism of Whitworth form is that it's too complicated. In 1864, William Sellars in the USA developed a simpler alternative; he realised that flat peaks and troughs (rather than rounded) would be easier to make, and moved to a 60 degree thread rather than Whitworth 55 degree. Simplifying production became a feature of all general-purpose thread forms designed after about 1870, including BA and Metric systems, and 60 degree threads have become the norm. WW2 finished Whitworth; it was first eased out in favour of UNC and UNF, which in turn are giving way to metric.

Actually you don't have to follow the Whitworth specification exactly to make a bolt that will fit a Whitworth nut. As long as the thread has the right pitch and clearance, the exact form isn't critical. I've seen genuine Whitworth nuts and bolts that are crude approximations. The point is, when cutting threads at home, it's rarely necessary to get them exactly right. (There are exceptions!) A common technique is to cut V threads nearly to size, then flatten the peaks slightly with a file, before testing fit with a nut. The thread is deepened slightly until the nut screws on, job done!

Couple of observations about screw-cutting on a lathe:

• Imperial threads (defined in turns per inch) make it easy to keep place with a Thread Dial Indicator, and complicated to work out diameter and depths. (Usually done by looking it up rather than doing the sums. For example, for UNC/UNF 60 degree threads, 1/tpi * 0.6134 (Whitworth is 55 degrees)
• Metric threads (defined in pitch) make it easy to work out diameter and depths, and tricky to use a Thread Dial Indicator. For that reason it is common to cut metric threads without disengaging the leadscrew. For M4 0.7, the rod is 4mm, and the depth of cut is the same as the pitch.
• Beware of winding the tool-post into the chuck under power while screwcutting! To avoid damage I usually cut threads left to right (thanks to JasonB), so that the saddle always moves away from the headstock.
• After a while you get used to cutting threads.

Dave

 

 

 

 

Edited By SillyOldDuffer on 21/06/2018 10:19:00

[David Standing 1Participant @davidstanding1]

Posted by SillyOldDuffer on 21/06/2018 10:18:09:

Posted by John Hilton on 20/06/2018 08:21:11:

…

My apologies for these questions – I expect it is all blooming obvious – but not to me yet.!

Thanks in advance.

John

• Beware of winding the tool-post into the chuck under power while screwcutting! To avoid damage I usually cut threads left to right (thanks to JasonB), so that the saddle always moves away from the headstock.

Dave

Now that is a good tip!

I bet threading left to right is counter intuitive to most of us, but it does make sense.

[Anonymous]

I screwcut a lot of (mostly imperial) threads. For standard V-threadforms I use full form inserts. They're not that expensive (probably cheaper than a quality die) and I buy them as needed. Full form inserts create a proper thread without having to waste time mucking about with files and dies. And if the thread pitch/diameter is non-standard there won't be a die available anyway.

I start with the material at the nominal thread diameter. Thread depth comes from tables. The theoretical values work pretty well, although I normally check fit against the mating part, or a test piece. A quick pass with a small brush helps to get rid of fine swarf, which can give a misleading impression of fit.

Can't say I've ever needed to cut a RH thread by traversing away from the headstock, but of course my lathe does have an automatic trip when screwcutting. Presumably one also has to reverse spindle direction as well?

Here's an example of a screwcut standard thread (3/8" BSP) and a non-standard one, 1" diameter 32tpi Whitworth:

Andrew

[larry phelan 1Participant @larryphelan1]

Hi John,

If you are like me and know as much about the lathe as it knows about you,fear not,you are in the right place.

These guys have forgotten more than we will ever learn,but to start off with,you need to get a simple thread profile gauge like the one shown above [you need this anyway if you want to grind your own tool bits ]

For the rest of the info,you could do worse than look up Sparey,,s book where he gives all the knowhow on thread cutting,in simple terms,no nonsense. Thread gauges are available to measure and identify different threads. they are quite cheap,and really,that,s all you need. Forget about getting bogged down with masses of tables and such,at this level,they dont really matter,your threads will turn out fine [even mine do !]

As one member said,a lick with a wire brush works wonders.

Now multi start threads are a different matter,but that,s for another day another time perhaps?

Give it a try,you might be surprised,I was !

[Author]

Posts