What's new
What's new

Repairing threads - take off .003-.004 mor on PD

SeymourDumore

Diamond
Joined
Aug 2, 2005
Location
CT
Guys, I have been handed a bit of a miserable job

Customer gave me 17 pieces of a fairly expensive part with a 1.5000-12 UNJF OD thread, which are just above high limit on the PD.
They are all about .0002-.0004 above. No more, no less.
Parts were gaged using a tri-roll for both PD and functional, and all readings show the same and consistant.

My question: What would be the best way to repair these?
I do not have any CNC equipment that can re-chase threads and never had to try and pick up an existing one and follow it.
I do have a manual lathe with threading, but WILL NOT go there as it is far far clapped out for this job.

So, my question is: Would there be an easy button for this job?
I am thinking of contacting a thread grind shop tomorrow. The parts are expensive enough to warrant a ground thread repair, assuming they have an easier
ability to pick up threads.

Thanks
 
Two to four tenths? Yeah, that's a grinder job. I'll bet these parts don't have usable centers, either, so job setup is going to be an OCD chore...
 
Ive chased them on a CNC, even one without the Thread pick-up option thingy. Just watched it close, stopped it, offset, rerun, stop, offset, rerun-ad infinitum.

It's as time consuming as it sounds, but it's doable for sure. Hopefully what you are Chucking, is Concentric to the Threads and doesn't need some fancy shim work. I don't know, but I would guess that a Grind shop is still going to have to go through all the same BS to get it right. I've never heard of them having any more magic than us. :D

But with the "J" there you have a little more wiggle room for a good blend. As opposed to a sharp Root, that requires more time to avoid Truncation.

Robert
 
I'd also be concerned about accuracy of the pitch, if you have a long enough thread and are not using the same machine for repair there could be a slight pitch error that shows up in a long enough section.

Aside from that, watch for lobing if previously done using a live center that didn't have a perfect point concentricity, general TIR on setup, not inducing heat damage due to improperly dressed grinding wheel (if grinding), and the obvious one - was the measuring lab temperature correct? The shop too, during the recut.

What's the material?
 
The parts are .0002 above max, so they can take off as much as .004 and still be OK.

I was thinking that thread grind shops might also be in the business to re-grind existing threads either to repair an otherwise messed up thread, or the under grind ( say ballscrew )
and the re-fit with a smaller mate if the cost warrants it.

Accurately locating however ... well that's another thing here.
There is an accurate through ID which was finished ( or so I was told ) in the same chucking as the thread, so perhaps an expanding mandrel would work.
 
Phuck that! I'd say you want to contact a thread grinding outfit. My guess is they'll piss n moan about the 2 to 4 tenths a bit before doing a pretty good job on it. Gonna be a crap shoot at best if on a lathe.

Brent

Edit: OK I now see they are 2 to 4 tenths high outta tolerance. Still isn't much wiggle room. If you're willing to eat a couple I suppose you could give it a go at the lathe. Grind shop be the ticket in my book. Good luck!
 
They are .0002” over, but that isn’t the tolerance. Sounds like .002” would get you centered. These should be possible to rerun on a cnc.
 
Grind shop seems good/best.. I have made a gauge nut with using rouge and a closure screw for a tight but close Acme and that worked for .0001 and a little more...perhaps .0002 or more in some areas..
 
With that little material needing to be removed I'd be making an adjustable nut out of bronze or CI to use as a lap. Just carefully size the minor dia. of the nut so it works all the way to the bottom of the external thread. Unless the threads are really long, it shouldn't take much to remove a few tenths.
 
What are the parts made out of???

1.5" J thread.. I'd guess something that is no fun, and probably in the stainless family. A286, 13-8 etc...

If it is some form of NON-stainless, I'd be tempted to toss them in some form of acid for a bit.. Maybe even some
vinegar for a few days...

J thread.. Controlled root radius.. And its tight. 15 to 18% of the pitch. .0125 to .015... two and a half thou
on the root radius...

My inclination, and I might be wrong since I've never had to do this... Send them to somebody that does thread rolling..
Shouldn't be a problem picking up the thread, the dies should take care of that.. Give her a little squeeze,
maintain the root rad and be done. That tiny bit of squeeze *shouldn't* effect the major much, but should get you in.

Next up.. Thread file, and F'it.
 
With that little material needing to be removed I'd be making an adjustable nut out of bronze or CI to use as a lap. Just carefully size the minor dia. of the nut so it works all the way to the bottom of the external thread. Unless the threads are really long, it shouldn't take much to remove a few tenths.

It's not unreasonable, but you may want to get confirmation with the customer that this is acceptable. If there's any risk of material transfer or remnant abrasive embedding, this could compromise the function of the part.

It has a "J" thread form, and these are usually found in high-load or aerospace applications. It's one of the reasons I asked about the part material (still unknown).
 
Is the part of such a design that you could thread mill the threads? It seems to me like you'd have a better chance to build a fixture and a 'part setter' that would load the part in the correct place to tickle cut it. Maybe even probe it somehow.
 
What's the material...
Well whadda'ya think!

Inco 625 of course!

If I had the right equipment, I'd probably give it a whirl.
I do have the option to trade some time at a neighboring shop on their toolroom Hardinge, but I am nervous about the part slipping
on the expanding mandrel.
Yes, if I just hit it for a .0005 DOC it would be all there, might go that route if the grinding shop says no.
 
Yeah, expensive materials, expensive part, critical application?

IMHO - find out what this dang thing is for, if aerospace (you are in CT, after all) it needs to be handled properly, which means paperwork and traceability. If for chemical industry, a little less stringent, but you still want to do it right.

I'd grind it, and look for a facility with the right capability. Get some feedback from whoever gave this job to you, and make sure it can be processed right.

Pray tell, why didn't it go back to the originating shop?
 
That's curious - someone posted about trying electropolish, but when I tried quoting it turns out the post had disappeared in that brief period.

Well, whoever posted that, it's a very interesting idea. Rather than the .0005"/surface suggested, I would just go for the barest minimum (2-3 tenths) to get the threads in spec, and yes, perhaps mask off the other surfaces.

But again, I'm concerned about what's acceptable for these parts and their application, I would still want approval from the end user before trying anything like EP or lapping.

And like this recent thread: https://www.practicalmachinist.com/vb/general/electro-polishing-354270/ shows, things can go wrong with EP, you don't want to wreck the parts.
 
First...I'd let the customer know there is a good probability of these parts becoming scrap. I wouldn't put myself on the hook for 100% job completion sucessful, and be the one to have to replace them if they do go south. Also, interested as to why he doesn't send them back to the vendor that made them for them to repair/replace.

It is possible to retrace in a CNC Lathe. Each part will be a one off though, and will require patience and time. This would be expensive to to, but possibly doable. "Stinky Inky" workhardens at cuts that slight, so you'll need to be cautious, and you may go through inserts fairly fast. You may also encourage the customer that .002/.004 over the high limit is still a functional thread when mated to a part...not so much a gage. A deviation could be considered with a reasonably intelegent customer.
 
I absolutely second what Derek Smalls said: this sounds like a quick lapping job to me for sure. The errors involved with grinding a part like this (both runout to fixture datum and picking up on the existing lead) seem like they make this a far more involved task than lapping the parts.
 
With that little material needing to be removed I'd be making an adjustable nut out of bronze or CI to use as a lap. Just carefully size the minor dia. of the nut so it works all the way to the bottom of the external thread. Unless the threads are really long, it shouldn't take much to remove a few tenths.

I've lapped tight threads for years. It takes a few minutes, but it works well.
 








 
Back
Top