Chasing (recutting?) external threads in 4130

[John Spangler]

Hi

Not a Mastercam problem, just a shop problem here.

We have a batch (3,600!!) tubes that were not threaded correctly, and was wondering what the best method for chasing the threads, and salvaging the parts was. Luckily, these were run before I got here, so I just get to FIX the mess, not get blamed for it, LOL.

 

Anyways;

Specs- 4130 Cro Mo tubing, External thread 1.125-20, threaded about .600 on one end of the part. Tube body is tapered on the other end. Aprox. 12" long. Wall thickness about .100

 

Any ideas what YOU would do to fix these?

 

Thanks

John Spangler

[GoetzInd]

So you just need to time the threads on a CNC lathe I'm assuming? How much under is the pitch dia.? That will dictate how much timing error you can have.

 

Mike

[crazy^millman]

My first thought would be to Thread Mill them. Make a Master locator block to locate the parts on the threads. Then once located to where the thread needs to be using an outside sliding block clamp in place on the mill. Then remove the sliding blocks that will time and locate the threads and then go to town. I could draw you something up if you would like. On a Lathe not going to be easy since hard to make sure it always times to the correct place. I think you would spend more time trying to line it up, verse going to a known set way on a mill where you can better predicate what the outcome will be. They are short enough to run on most standard CNC Mills. Trick will be having the operator pay attention to the bottom of the parts to make sure he bringing them all up to the correct place when lining them up to the sliding block. You could also do a small cut out in the sliding block so you can see it has bottom out correctly every time. In the long run might be cheaper just scraping them out than the probably 1 minute per part it is going to take to re-machine them. Fixture would I think take about 6 to 8 hours to make and set-up. Using a multi-flute carbide threadmill will help, but no where near as fast as a lathe.

 

Second thought if you got a mill turn then it could get very interesting, but I still worry about the lathe always picking up the thread in the same place every time. Maybe with a C axis lathe and a block with threads on it put in a turret location you then thread to to align it would work, but it would take some trial and error before you got it dialed in and your lathe better be top notch.

 

Third thought thinking about it more as I type this I guess you could try the same thing on a regular lathe would just need to be half of the thread female cut into a block to come down from the turret. Bring the turret down in X to a know Z. Make sure the jaws have almost no movement when clamping down on the tube maybe collet if you have it. That should align the threads to the same place every time and then once you dial in the thread cycle it might work, but my safest best is a milling fixture.

 

HTH

[Pilot Plant Supervisor]

This is where an old school Geometric die head is still of use. Set up on a manual lathe or turret lathe and go to town.

[GoetzInd]

This is where an old school Geometric die head is still of use. Set up on a manual lathe or turret lathe and go to town.

 

That's what I was thinking but not too many people have them and they aint cheap.

 

Mike

[John Spangler]

My first thought would be to Thread Mill them. Make a Master locator block to locate the parts on the threads. Then once located to where the thread needs to be using an outside sliding block clamp in place on the mill. Then remove the sliding blocks that will time and locate the threads and then go to town. I could draw you something up if you would like. On a Lathe not going to be easy since hard to make sure it always times to the correct place. I think you would spend more time trying to line it up, verse going to a known set way on a mill where you can better predicate what the outcome will be. They are short enough to run on most standard CNC Mills. Trick will be having the operator pay attention to the bottom of the parts to make sure he bringing them all up to the correct place when lining them up to the sliding block. You could also do a small cut out in the sliding block so you can see it has bottom out correctly every time. In the long run might be cheaper just scraping them out than the probably 1 minute per part it is going to take to re-machine them. Fixture would I think take about 6 to 8 hours to make and set-up. Using a multi-flute carbide threadmill will help, but no where near as fast as a lathe.

 

Second thought if you got a mill turn then it could get very interesting, but I still worry about the lathe always picking up the thread in the same place every time. Maybe with a C axis lathe and a block with threads on it put in a turret location you then thread to to align it would work, but it would take some trial and error before you got it dialed in and your lathe better be top notch.

 

Third thought thinking about it more as I type this I guess you could try the same thing on a regular lathe would just need to be half of the thread female cut into a block to come down from the turret. Bring the turret down in X to a know Z. Make sure the jaws have almost no movement when clamping down on the tube maybe collet if you have it. That should align the threads to the same place every time and then once you dial in the thread cycle it might work, but my safest best is a milling fixture.

 

HTH

I like the third Idea. Not really following the first, but I'll repeat it to the boss to sound smart!!

 

It seems like the od was left big when these were threaded. The problem was that the customer supplied the mating part, with no prints, etc., only

a sample.

Thanks

john

[crazy^millman]

Well hopefully it is helpful and just give you some different ways to think about it. Thing is I had to do this same thing for a company years ago and with no lathe I only had the mill to fix them.

[jeff]

That's what I was thinking but not too many people have them and they aint cheap.

 

Mike

 

I think we have one somewheres

[Guest MTB Technical Services]

If re-cutting threads is something you will do on a regular basis,

it's worth considering getting a Weiler lathe.

 

Hands down, simply the best lathe on the planet for re-cutting threads.

Only takes about 30 seconds to pick up the thread lead and you're ready to cut.

http://www.mtbtech.n...-by-Weiler.aspx

[taperlength]

Something similar to CM's idea. Make a ring gage that fits the bad parts. The gage should be longer than the thread and have a counterbore Then take a scrap piece of tube, put it in the chuck of your cnc lathe so that it sticks out exactly the same length as the gage you just made and cut a thread the same as the bad parts. Without taking that part out of the chuck, screw the gage onto the scrap tube so that the end of the gage is flush with the end of the tube. Then make matching punch marks on the outside of the gage and the chuck jaws. After that, you should be able to load any tube into the chuck and time it exactly the same as the setup part.