Threading a leadscrew with a lathe

[MrRage]

Is this a good idea or not? I wanted to get a new leadscrew for my milling machine and thought that maybe I should just try using my lathe and make one instead of buying it.

My main concern is accuracy. I just need to precision thread up to 16”. The lathes is a 10x24” lathe so it can handle the capacity, but is there anything I should know before I try this?

[Razor]

Hi MrRage
It certainly is possible but you need a suitable lathe (with the correct gearing - to ensure you can create the right tpi) Correctly ground tooling and some skill.
Good Luck
Razor

[Stevie]

you'll need a traveling steady rest; to keep that length from flexing away; the best material would be UHMW for the pads

[MrRage]

Here is a picture of my lathe. Its an enco belt driven model, 10x24". I'm cleaning it up right now because the previous owner neglected it. So a traveling steady rest would help this operation, I’ll have to look into getting one.

http://epyon.54.org:8000/~dustin/workshop/Lathe.jpg

[HuFlungDung]

Actually, carbide pads would be better on your travelling steady. The rough burr that can occur at the top of your threads as you cut them, will just chew up UHMW or even brass pads. When using soft pads, pretty soon, they will wear in and act like a 'half-nut' and want to keep feeding your carriage along. Ask how I know this

Having said that, a nice machinable screw stock to use would be Stressproof shafting, because of the sulfer added to this alloy, it makes it a very short chipping material.

[MrRage]

What if I were to setup my lathe with an angle grinder that had a decent grinding wheel attached to it and used that to cut the threads instead of a cutter. Or would something like this be better as a finishing operation?

I’d have to fabricate a specialized bracket to hold the grinder, or might even have to use a bench grinder instead because of the forces involved. But I would think the outcome would be better if I were able to pull this off.

[Razor]

Hi MrRage
The angle grinder sounds dangerous to me. The proceedure of cutting threads on a lathe is quite common, in fact this is how a toolmaker would make a thread as it gives a much better result than screwing a thread die on the rod.
Starting point: have you got a suitable lathe. ie can it move the tool along the lathe (rod) at the correct distance per revolution of the chuck to give you the TPI that you want? Does it have a suitable tool holder?
Next: Grind up a HSS tool bit to the exact shape of the thread you are going to produce.
Then report in
Good luck
Razor

[Stevie]

I suggested UHMW as throw away pads; do one job and thats it; it's cheap and who cares if it wears
Cut a Square thread first; then use a thinner Acme profile for the flanks; use reverse to return to the start point; don't disengage the leadscrew nut
actually reversing will most likely remove and gouging the screw will make in the UHMW; just try to maintain and even pressure with the pads so as not to push the material into the tool
Thats how a "real" tool and maker would do it; how do I know; because after 36 years as one; I feel I do know

For a home project Carbide pads would be a bit too much money; they would need to be type specific for the steady rest

[Stevie]

What if I were to setup my lathe with an angle grinder that had a decent grinding wheel attached to it and used that to cut the threads instead of a cutter. Or would something like this be better as a finishing operation?

I’d have to fabricate a specialized bracket to hold the grinder, or might even have to use a bench grinder instead because of the forces involved. But I would think the outcome would be better if I were able to pull this off.

I manage a custom grinding shop; I would never let one of my guys do anything like this
Right tool shape; right material; good tapping compound like Rapid tap; and it will look like factory
I built a small toolpost grinder for the shop; it works great for small holes and the odd job we can't get into a real grinder; but trying it on threads "not a chance"

[Mcgyver]

I've cut long acme threads (actually for a mill feed screw) and you can get an good results on the lathe. The accuracy will be that of your lead screw, which on a good lathe is a precision ground screw. Like Stevie says you will need a traveling steady. I found you also need a bit of a feel as the force you apply with the steady (to hold better than a thou over a couple of feet) changes as the lathe comes away from the tailstock/approaches the headstock.

I've never used plastic on the steady but would be concerned about compression or wear. Mine has bronze pads and maybe over a lifetime they'd wear out, but the are sacrificial and didn't seem to mind the job. If there is a burr that will wear them, it should fall in the same place with the same spot and the pad itself will be in the same position to the crest of the thread with each pass (or knock it off by following the following rest with a file). HuFlung makes a good point that the pads will wear to, and start to act like a screw - using harder bronze and lightening up on the pad pressure towards the tailstock will help, run the lathe in the lowest speed and be ready on the stop button.

Not disengaging and running the lathe in reverse would be tedium, but if you have no half nut that is what you have to do, (although for roughing I'd just manually position it)

I completely agree with Stevie on the grinding. Grinding is a finish op and thread grinding is not something I’d want to try on the lathe. you would never get a good result trying to precision grind with bench grinder - the bearings are to sloppy .

You’ll need an acme thread grinding gauge, getting the right form cutter is half the battle. I used, and would recommend, a free cutting steel. The width of cut on an acme thread is huge, and this is already a flimsy set up. If this is too soft, then you are probably doing it for industry in which case you should buy ground threaded stock or have it made hardened and ground.

Alternatively you can cut the acme thread in little chunks, kind of like if you divided up the thread profile into squares like graph paper and cut out a square with each pass. This will reduce the cutting force but would be a pita.

So long as you stay away for crazy grinding ideas, the worst that’ll happen is you’ll learn a bunch and mess up some lengths of steel, so go for it.

[Stevie]

[QUOTE=Mcgyver]

I've never used plastic on the steady but would be concerned about compression or wear.
Not disengaging and running the lathe in reveres would be tedium, but if you have no half nut that is what you have to do, (although for roughing I'd just manually position it)


QUOTE]

I'm not sure his experiance level will allow him to be disengaging the lead nut; while it's slower to some; if you run at the speeds i thread at is no different than winding it back by hand
If you had tried UHMW for pads i doubt you'd go back to bronze

[Geof]

Having made both small acme screws, 1/2" diameter 14 inches long (see picture) and large, 1-1/8" diameter 30 inches long (sorry no picture) I was going to say it is possible, but probably not as precise as you would like and unless you are doing it for the satisfaction of meeting a challenge, probably not worth the effort. However, all the experts have weighed in so I will simply recount my experience and not make any suggestion either way. I found that while my small lathe had a fairly good leadscrew, significant inaccuracies in the machined thread arose from the poor quality of the gear train between the spindle and leadscrew. On the smaller diameter screw it was a real pain avoiding chatter. I had a purpose built travelling steady with a fully hardened steel bushing and the chatter was not coming from the material deflecting radially, but from torsional deflection; nothing at the chuck and, unless very light cuts with only a partial form tool were used, intolerable at the free end. On the larger screws my poor little lathe bogged down trying to use a full form tool and these screws also needed several partial form tools. It also took a long time, I seem to recall the small screws started at around an hour each and never came in below 35 minutes. Eventually I built a semi-automatic threading machine where the operator was only responsible for loading and the tool in-feed; nut engagement, disengagement and carriage return were automated. This brought the time down to 7-1/2 minutes just for the threading. The screw in the picture was done on a Haas HL1 with a purpose built steady rest, parted off from bar stock at about 5-1/2 minutes each.