How do you cut multiple start threads?

I have cut threads from time to time, certainly no expert. And I have studied a lot of old books on machining. But this is something I am confused about. How the heck do you cut say, a 4 lead 2" diameter acme or square thread?
The latest toy many blacksmiths are into these days is a fly press- a manual press, with a 4 lead thread, and two big round weights on top, for hot and cold forming. There used to be jewelry factories in Rhode Island and Ct. with hundreds of these things in em, but my guess is they are all toyota's now, as there are two different companies importing new ones from India- probably Atlas products.
But being cheap, blacksmiths want to make their own- and want to cut their own 4 lead threads on their 6" atlas lathes.
Seems like even with a CNC lathe, multiple leads are tricky. How did the oldtimers do em on a manual lathe?

I set the compound to 90 degrees. Then cut one thread, using the thread dial normally. (There was a good thread in here not long ago about threading dials if you have any question about that.)

Then, crank the compound along 1 thread pitch and cut another one, repeat a similar procedure for all the threads.

When cutting Acme or square threads, it is beneficial to be able to jog the compound back and forth a few thousandths for alternate cuts, to keep the chip from jamming in the threads. I know this adds to the complexity, but you just have to keep the proper setting (on the compound dial) in mind as you do this. Use a roughing tool that is narrower, to avoid a screw up in cutting overwidth. When all the threads are roughed, then start over with a full width finishing tool and feed (incrementally) straight in, with the compound set in one position only, for each individual thread.

Hi Ries:

If you get to look at some of the older lathe catalogs you will see sub head stocks were offered. This was nothing more than a gear box clamped to the ways just in front of the spindle nose. Usual ratio was 6 to 1. The old slow lathes were six times slower with this thing in action.

Mostly intended for use with relieving attachments, but also for long lead thread cutting. I.E., if you set the QC to 10 TPI and had the SH in place, you would cut a .600" lead thread.


Best I ever did without a sub headstock was nine start 7/8 dia with 1" lead. For breechplug that unscrewed down thru barrel (by going around with trigger guard) to open up breach for loading. (Someone's Rev. War era patent, but I don't recall who.) This did not work, since no one got around to making mating ID thread, but it was neat to look at.

You really have to pay attention to tool geometry when things stretch out this far. The cutting tool has to be ground so it lays over to match helix angle of lead.

What is really fun is trying to make the mating nut!

I have seen lathes geared for long leads where it became necessary to drive lead screw instead of spindle, just so the gear train would not break.

John

A 2" 4 start acme just ain't gonna happen on a 6" atlas unless its the world's finest pitch thread

To cut any multi start thread on a manual lathe, you'd first need to set the compound parallel to the ways instead of at the normal for threading 29 degrees. Lets say you want to cut a 4 start 16 tpi thread. You'd set up your gearbox to cut 4 tpi. Zero the compound, and cut the thread to full depth. Advance the compound one pitch (1/16") and cut another 4 tpi thread. Advance compound another 1/16" and cut the third thread. Advance another 1/16 and cut the 4th and final thread. All infeed is done with the cross slide, but by advancing the compound .001 for every .005 or so of infeed, its still possible to do V thread cutting on just one side of the tool like you would with the compound at 29*. An acme would be pretty much the same drill, except that you'd have to calculate the compound feed to properly correlate with the angle of the acme thread. A 4 start 10 tpi Acme would require you to have the gearbox set for 2.5 tpi. Thats where the main problem comes in. Once the part is turning at a decent surface speed, the threading tool is hauling ASS toward the chuck.

Cutting them on a turning center is relatively easy. Some have parameters that you set to spec multistart, and on the ones that don't, all thats necessary is to alter the Z offset by one pitch each time and run the cycle 4 times ( for a 4 start). The main thing you have to verify when doing them in a turning center is that you have adequate clearance on the tool for the high helix angle. This applies to manual threading too, but is easy to forget when doing them via CNC since the rest of the job is so easy.

WOW !

Two very well-written explanations, dovetailing perfectly and composed simultaneously. (Twin sons of different mothers, or something like that ...... mumble, mumble)

edited to add:

THREE well-written explanations, all at virtually the same time!

Gentlemen

Only has cause to cut a few multi start threads.
Whilst I’d concur on the above methods to produce the offset between the flights of thread with the compound slide.

When I was an Apprentice we were shown another method, it only works for shafting between centres. That was to have a multitude of drive pins on the face plate. Two pins at 180 degrees for 2 start, 3 pins @ 120 degrees for 3 start, 4 @ 90 deg for 4 etc.

You would turn and finish one helix of the thread, then remove from your centres and move your drive dog to the next pin. (Never unclamping the drive dog from the work). In essence rotating the work in relation to the spindle and feed train position.

That allowed you to have the compound slide at an angle if that was your preference, or to take side cuts on the flanks.
And if the drive pins were accurately layed out by co-ordinates on the face plate. Indexing it with this method was said to give excellent tolerance from start to start, and less confusion with keeping up with your compound dial position.

Just another way to skin a cat.

Regards Phil.

Agree with everything said here, especially the part about this not being possible on a 6" Atlas. The 24" Pacemaker at work will only cut a 1TPI.

The Hendey catalog I have shows how to set up for multiple lead threads, using the sub head (6:1 as has been mentioned) with a "dividing faceplate". This is a driving plate for a straight tail lathe dog. It has a number of holes, set up kind of like a dividing plate for an index head or rotary table. A ring of three, four, and six holes would be most likely.

The work is mounted between centers and the dog is clamped in place. The dog is not moved on the work during the process. You start your first thread and cut to depth, move the stud to a hole in the ring of holes you want to use and start threading again, with the thread dial at the exact same place. You have indexed the position of the dog, so the work has indexed around for the next lead.

Very good explanations, but I was wondering, what is the real advantage or usefulness of a multiple start thread? What are they typically used for?

They're used when you want a lot of travel per revolution of the screw, but don't want some monstrous coarse thread to get there. In the example I posted above, you'd have essentially a 16 pitch thread, but every revolution of the shaft would make the nut move 1/4 inch. In this instance the pitch is 1/16 (measured from crest to crest of adjacent threads just like a single start), but the lead is 1/4 (measured from crest to crest on ONE thread)

I'm *almost* certain that Ries was pulling our leg about the 6 inch Atlas.

Think of multiple start threads in applications where cams might also be useful. It's a neat way of translating angular motion to axial motion, fairly simple to produce and with greater strength than single threads.

(As mentioned above, sometimes used in firearms of large caliber.)

Another way to cut the multi-start is to rotate the spindle in relation with the first idler in the gear train.

You'd have to mark the spindle gear at four equally spaced teeth, as well as the idler on one marked tooth at the spindle gear.

Cut one lead.

Set spindle with two marked teeth matching, disengage quadrent and rotate spindle to the next mark.

Re-ingage teeth, cut second tooth and continue as above to complete the job.

When I was an apprentice boy we marked one chuck jaw. Than drilled and reamed four holes equally spaced on a plate fitted to the job with a setscrew.

With a pin in the first hole against the jaw, cut one lead.

Rotate the job with the plate to finish the cuts as required.

Quick and dirty.

kap

machtool, seems you must have been posting as I was finishing up typing!

Agree with all the above posts. I have another method on a lathe at work. The machine is a 21" "Dong Yang" (Okuma liscence made in Korea and very nice) The spindle nose is marked off with a zero and numbers 1 through 6. There is a reference line on the headstock. Here is how it works: start the job as a normal single lead thread and cut as usual with the compound at 29 degrees as usual. when the first lead is fininsed you put the gear for the headstock in neutral (to turn it easily by hand) and rotate the spindle forward to the "0" is aligned with the index mark. Now you disengage the feed reverse lever and advance the spindle forward to the number on the spindle that is equal to the number of starts you need,say "4". Line up the number "4" with the index mark and re-engage the feed reverse and begin cutting your next lead...
Works pretty slick.
Cheers Ross

I was indeed kidding about the 6" atlas. But there are always those guys out there who want to do something like that.
The specific application is for a fly press, which is a tool that a 4 lead thread is perfect for.
I have no intention of building my own fly press- if I want one, I will buy a cheap Indian made one.
But I have always wondered about the multiple start threads, and now I have a much better understanding of it. I will probably try doing one, on my 18" x 60" lathe, not an atlas, just for the halibut.
As I said before, although the existence of it is casually mentioned, none of the dozen or so books I have on running a lathe actually goes into the detail of how to do it.
PM comes thru again.

WOW...you guys are working WAY too hard.

Using a Lodge and Shipley lathe I just use the threading dial.

I set up the threads for whatever...if its a double lead 6 then the gearbox is set up for 3 TPI. I then use the threading dial to cut each lead, and I'll do each lead at the same time. I'll usally mark the threading dial with a magic marker to keep track of the numbers on the dial and the lead that they correspond to.

Its quick and easy. I use a thread stop for the carriage feed and use the compound set at 14.5 and use it to advance the tool into the cut.

I do alot of double and occasionally a triple lead for ACME threaded valve stems and nuts.

BobB:
That only works if you are cutting a pitch that is an odd number dosen't it? If you are cutting even number threads dosen't the same thread come up on any line or number?
Cheers Ross

Mike C.

Lets just put that down to “Great minds think alike” That happens to me all the time, as I write my stuff in word, then cut and paste it into the reply box. That can take me 20 minutes some days if I get a few interruptions or have to think about it some.

I’m forever, getting “piped at the post” by a few minutes or so.

I went looking for my face driving plate this afternoon. I’m sure I used to have an indexing drive plate for my lathe. Can’t find it any place. I think I adapted it for a new chuck. That’s how many multi start threads I cut. I’m sure the last one was a machinist’s jack when I was an apprentice.

Regards Phil.

alfpha,
I think you're right.
kap

I made some water glass valve stems and glands when I worked for the railroad. The stems were a piece of cake. I turned up a center in the 4 jaw chuck and cut the threads between centers. Alternating between 2 jaws 180 degrees apart for indexing.

The glands were set up on the "indexing" faceplate. We had a chuck bolted to the faceplate and the threads were machined by indexing 180 degrees between cuts...They were 5/8" or 3/4" diameter with I think an 8 pitch...

I have some tubes to make for some kind of scientific sampling instrument in the next couple of weeks. Good timing on this posting.

Andy Pullen

The brain is a terrible thing- once you turn it on, it just keeps going...
So I get it now, but of course this only brings up more questions.
In a semi-production situation, wouldnt it be easier to cut a multiple toothed lathe bit, and run all the leads at once? No misalingment potential between leads, equal depth of cut, equal angles on every one.
For a bigger size, say 4tpi, you could just gang together ground down tool bits.
I realize for real manual mass production, you would use die heads, but for single point cutting, it seems like multiple point cutting would be pretty efficient.

Which brings me to my next question- when you say, "cut the thread to full depth", how do you know what that is? For matching an existing piece, or a repair, I get it. But where do you find industry standards for multiple threads? If it is in machinery's handbook, I sure cant find it- they pretty much just acknowledge that multiple start threads exist. But where are there published standard sizes, thread profiles, etc?