Metric Thread Forms

[kiwi2]

Hi,

I've been cutting threads on a lathe for years in a rough and ready way. I keep removing metal until a nut will just about go on and finish the job with a die nut. I needed to cut an m8x1.25 thread today and decided to calculate the infeed required on the compound slide and do the whole job on the lathe.
Initially I assumed the thread would take the form of an equilateral triangle with the base dimension being the pitch. The result I got was way off so I've been looking at the actual metric ISO thread form (see the photo).
I'm a bit confused now. In the past, if I wanted an m8 thread I would have started with an 8mm diameter rod.
From the look of the ISO thread form, it looks like the distance H can be calculated to be the pitch/2Tan30 = 0.866 x pitch. For a 1.25mm pitch, this works out to be 1.08mm.
The crest of the thread however is shown to be H/8 below the apex which again, for a 1.25mm pitch works out to be 0.14mm.
My question is - If I want to cut an m8 x 1.25 thread, should I start with a rod of 8.0mm diameter, or should I start with a rod of 8 - (2 x 0.14) = 7.72mm?

Thanks,
Alan C.

 

[Wizard69]

That is a good question!

In most cases where I tried to start a die on full size rod it has been a physical battle even after cutting a chamfer. I haven't done so lately but if I remember correctly the die shaved off the apex. This by the way was unified thread but I don't think there is a hug difference.

In any event this is a good place for a little research. Try threading one stud at nominal diameter and the other with the shafting turned to the dimension you referenced. In the end I suspect the threads will be very similar. However the shaft you turned down should thread a lot easier if you use a die. By the way I suspect that it is hardly noticeable at smaller diameters.

As an aside pick up most bolts and measure the thread width and I think you will find the diameter of the threads to be slightly below nominal.

 

[Hopper]

It is usual to machine the stud to slightly undersize before commencing screwcutting. There has to be some clearance between the tops and bottoms of threads. I work in Imperial, so for an equivalent 5/16" thread I would start with the stud diameter measuring about .005" to maybe .010" undersize. So probably more like 7.85mm in your example.

Don't be afraid of making the stud OD too small. You can go down to about 65 per cent thread engagement before it seriously weakens the strength of the threaded joint. 85 per cent engagement is commonly aimed at. Your 7.72mm would be within that range.

Then it is usual to stone the point of the screwcutting tool to a small radius so you lose that pointed part of the thread.

Screw cut to the theoretical depth, checking for fit the last few cuts. Run a three-square file over the crests of the thread to clean off the burr before fitting.

Be aware that most commercially made nuts are made on the loose side, so start checking for fit well before the final depth is reached. If making your own nuts, or female threads in fittings etc, do them first and finish off the last little bit with a tap if you can. Again, the hole in the middle should be slightly oversize to allow clearance. It is easier to then machine the male thread to fit the existing female than the other way round.

If you really want to get into the nitty gritty of it, and learn more about screwcutting than you are likely to ever need to know, Martin Cleeve's little book "Screwcutting in the Lathe" is worth its weight in gold. It's Workshop Practice Series book so costs about $15 delivered to your door. You couldn't beat it with a stick.

 

[rodw]

Funny, I was looking at this too because I need to cut an M12 x 1 thread and dies are not readilly available for that one. On Wiki, I was reading that many thread forms are truncated by using an undersized rod. Any bolt I've measured are about 0.2mm undersize.

I have also read that the depth is 0.614 the pitch so I think that implies an undersized rod.

I was going to try on some 12mm rod and go to the full depth of .866 you quoted.

 

[Charles Lamont]

The leftmost dimension on your diagram, Dmaj, is your nominal 8mm or whatever.

The sharp crest extending H/8 above the nominal diameter is just a theoretical part of how the geometry is defined, not part of the actual thread. The
thread depth you cut is 5/8H, plus a bit for the tip radius on the tool.

In practice, cut until it fits.

A crest radius on the male thread is also allowed, within the profile shown in the diagram by the thick line, and normally rolled-thread bolts will have this radius.

 

[gbritnell]

There are two thread forms we generally use, one with a sharp V and the other a manufactured thread form which has flats and radii. A tap has sharp corners so therefore cuts with a sharp V. When cutting with a hand ground threading tool in the lathe it cuts a sharp V. When testing a lathe cut thread with a manufactured nut the nut has a radius at the root of the thread so sometimes there is some binding. It's always better to make the shaft slightly undersize if you are going to be using a nut on it. The mistake some people make when fitting the nut to a chased thread is they find that it's snug so they chase the threads a little deeper which is wrong, in some cases. The thread should be the proper size at the pitch diameter for a good fit. By chasing deeper in effect they are removing more metal from the outside diameter but also making the pitch diameter smaller and ultimately making a sloppy thread match.
Threading on the lathe with carbide thread insert tools will give the proper flat at the root of the thread but not with a high speed sharp V tool.

 

[rodw]

Well, I achieved what I set out to achieve

Not bad for my second ever thread. Now I hope everything fits up. If you are wondering, this is a spindle to fit a pair of ball screw bearings. So if it were a standard 16mm ballscrew, the thickest part would be the ballscrew thread.ONe end will have a pinion for a rack and pinion drtive and the other a timing belt pulley for a reduction drive frrom a stepper motor.

 

[Charles Lamont]

There are two thread forms we generally use, one with a sharp V and the other a manufactured thread form which has flats and radii. A tap has sharp corners so therefore cuts with a sharp V. When cutting with a hand ground threading tool in the lathe it cuts a sharp V. When testing a lathe cut thread with a manufactured nut the nut has a radius at the root of the thread so sometimes there is some binding. It's always better to make the shaft slightly undersize if you are going to be using a nut on it. The mistake some people make when fitting the nut to a chased thread is they find that it's snug so they chase the threads a little deeper which is wrong, in some cases. The thread should be the proper size at the pitch diameter for a good fit. By chasing deeper in effect they are removing more metal from the outside diameter but also making the pitch diameter smaller and ultimately making a sloppy thread match.
Threading on the lathe with carbide thread insert tools will give the proper flat at the root of the thread but not with a high speed sharp V tool.

I beg to differ. My taps are HSS ground, not carbon-steel cut-thread. They are in no way special, but they do not have sharp crests, but a proper thread form. For external screwcutting with a hand-ground HSS tool, I hone a radius on the tip. For screwcutting an internal thread I generally do leave the tip sharper.

 

[Hopper]

Well done RodW. Git 'er done, that's the way.

 

[Hopper]

Another old screwcutting technique that seems in danger of being lost in the mists of time is to set the topslide parallel to the lathe axis and then when you move the screw cutting tool in say 10 thou with the cross slide, advance it five thou with the top slide. This moves the tool in a direction slightly less than the 30 degree offset sometimes used. Thus, cutting is mostly on the leading edge of the V screwcutting tool, with a very light shaving by the trailing edge to eliminate any "stepping".

The advantage of this method is that when you get to the correct theoretical thread depth but your test nut does not fit on, or is very tight fitting, you can then use the topslide to advance the toolbit say one thou without taking any extra depth of cut. You then take a cut, clean off burr and fit the test nut again, repeat etc until correct fit is found.
You can also of course, retard the toolbit by a thou or so, allowing for backlash in the topslide screw by backing it off half a turn then coming back to the minus one thou position. This will take a tiny clean up cut along the trailing flank of the thread.

With a nicely stoned tool bit you can get a mirror finish on threads like this and get a perfect fit without going undersize on your diameters.
But it is a bit fiddly.

 

[kiwi2]

Hi,
I decided to follow Wizard 69s advice and try cutting an m8 x 1.25 thread using both a 8.00mm rod and a 7.72mm rod. I cut them both until a nut was a tight fit on them. The root diameters came out pretty much the same (calculated from the movements of the compound slide and the starting diameters) with the 8.00mm rod being 6.35mm and the 7.72mm rod being 6.33mm.
The finished threads are shown in the photos below.
The thread on the 8.00mm rod has sharp edges and doesn't seem to follow the ISO form.
The thread on the 7.72mm rod has a flat on the top as per the ISO form. I printed the picture and measured the flat using the pitch of 1.25mm as the scale. The crest is P/4 rather than P/8 as stipulated by the ISO.
I ran a die nut over each thread. As usual, the thread on the 8.00mm rod never really rotated freely in the die nut while the thread on the 7.72mm rod did.
The diameter of the 7.72mm rod was calculated from:

d = D - 0.222P where:
d = the reduced diameter
D = nominal diameter
P = pitch

I think in future I'll try:

d = D - 0.111P

Regards,
Alan C.

 

[goldstar31]

If you really want to get into the nitty gritty of it, and learn more about screwcutting than you are likely to ever need to know, Martin Cleeve's little book "Screwcutting in the Lathe" is worth its weight in gold. It's Workshop Practice Series book so costs about $15 delivered to your door. You couldn't beat it with a stick.

For those interested, I wonder just how many constructed the 'final' design of retracting swing tool holder which appears on the front of the book.

It serves the same purpose as the two variants in Thomas's Model Engineers Workshop Manual.

Me, I am merely curious as I have a fabricated 'original' tool to Cleeve's design

 

[gbritnell]

What is your point Charles? I stated that taps have a sharp V form. If a person wants to hone their tools to get the proper form so be it. I personally have never found it necessary.
gbritnell

 

[Charles Lamont]

What is your point Charles? I stated that taps have a sharp V form. If a person wants to hone their tools to get the proper form so be it. I personally have never found it necessary.
gbritnell

I did not actually say I am so daft as to try honing my taps. Where I disagree is that I am saying I don't think I have ever seen a tap with sharp crests. My tea is now cold because I have just been out to the shop and compared a 1/2"BSF tap with a 16TPI Whitworth-form hand chaser. The forms match as well as I can see with 12x loupe.

 

[james_III]

Over here metric world good starting point is 0.1mm undersize from nominal diameter. Sometimes it is not possible, so one fast filing push is needed to flatten thread a little. Metric normal thread is not the best there is but that's not the point.

Thumb rule for thread depth is same as pitch, witch works on normal cases. This is based on M6X1 dimensions, if pitch is more than 2.5 thumb rule will get inaccurate. There is no need to overcomplicate things :hDe:

 

[james_III]

The advantage of this method is that when you get to the correct theoretical thread depth but your test nut does not fit on, or is very tight fitting, you can then use the topslide to advance the toolbit say one thou without taking any extra depth of cut. You then take a cut, clean off burr and fit the test nut again, repeat etc until correct fit is found.
You can also of course, retard the toolbit by a thou or so, allowing for backlash in the topslide screw by backing it off half a turn then coming back to the minus one thou position. This will take a tiny clean up cut along the trailing flank of the thread.

With a nicely stoned tool bit you can get a mirror finish on threads like this and get a perfect fit without going undersize on your diameters.
But it is a bit fiddly.

More advantage and maybe more important this is way less power hungry method to cut thread with larger pitch.

 

[blighty]

good thread.....

i have always wondered this my self. i to tend to go the way of keep going in till the nut part fits. but some times you cant do that, as in you would have to take the part out of the lathe to the job to see if it fits. not a good idea.

looked in to it more when i had to cnc a thread on a lathe. on a run of parts i would do the same thing. make a part, see if it would fit. then adjust the g-code till it does. thats ok if your doing lots of small parts, but what if your doing big one. you need to know exactly how far you have to go in. I did find a formula that would work this out for you. think it was metric only. for e.g divide pitch of thread by 0.873542 kind of thing that would give you the DOC.

i'll have a look on the pc at home see if i can find it.

 

[blighty]

had a look on the old net and found this.

http://www.calcool.dk/metricthread.htm

looks like you would be right with 1.08mm

 

[mu38&Bg#]

I have just been out to the shop and compared a 1/2"BSF tap with a 16TPI Whitworth-form hand chaser. The forms match as well as I can see with 12x loupe.

That's expected as these thread profiles specify radii on crests and roots. They are not optional. Aren't these threads obsolete?

Virtually all standard 60° thread forms allow sharp roots and taps and dies are typically supplied this way.

 

[napoleonb]

It is my understanding that a radius induces strength for one and reduces the risk for metal-fatigue and stress-cracks.
Also there are min and max tolerances for fit and function, I've attached a table from an old book regarding threads showing the differences between them.