What's new
What's new

Thread Help! 2-1/2" - 4 UN

scrapped

Plastic
Joined
Oct 28, 2021
Hello everyone! I've used this forum as a source of info for a while and figured I'd come here for help on a thread.

Material: 1141
2.50" x 59.25"

Thread is a 2-1/2"-4 UN for a length of 28".

I'm having some vibration issues. Running a Hurco TM12i using this insert: Turner Supply | 5ER4UN Grade VKX Threading Insert

Any suggestions as to decreasing depth or rpm. This is the longest thread I've attempted on a CNC. Any help is appreciated.
 
A 4UN on 2.5" diameter over 28" (presumably) unsupported other than chuck and tailstock?

That's really pushing it, to the point that vibration is guaranteed, not avoided.

If you really have to screwcut it in the lathe, generated form with (much) smaller cutting edges is the get out of jail free card for this. That's not so easy though if you don't have cam that supports it, but it can be trig'd out and put in a spreadsheet for each pass...

Of course this will heavily impact your cycle time, so the quantity you have to do and the time allocated will determine if this is a viable solution.
 
Hello everyone! I've used this forum as a source of info for a while and figured I'd come here for help on a thread.

Material: 1141
2.50" x 59.25"

Thread is a 2-1/2"-4 UN for a length of 28".

I'm having some vibration issues. Running a Hurco TM12i using this insert: Turner Supply | 5ER4UN Grade VKX Threading Insert

Any suggestions as to decreasing depth or rpm. This is the longest thread I've attempted on a CNC. Any help is appreciated.

We can't make suggestions on speeds, feeds or tell you if you need to decrease your d.o.c. until you tell us what you're currently running it at.
1141 is a nice material to cut.
 
A 4UN on 2.5" diameter over 28" (presumably) unsupported other than chuck and tailstock?

That's really pushing it, to the point that vibration is guaranteed, not avoided.

If you really have to screwcut it in the lathe, generated form with (much) smaller cutting edges is the get out of jail free card for this. That's not so easy though if you don't have cam that supports it, but it can be trig'd out and put in a spreadsheet for each pass...

Of course this will heavily impact your cycle time, so the quantity you have to do and the time allocated will determine if this is a viable solution.

Yes, chucked with a tailstock is the only support. Jaws bored well, center is running dead nuts (thankfully lol)

We can't make suggestions on speeds, feeds or tell you if you need to decrease your d.o.c. until you tell us what you're currently running it at.
1141 is a nice material to cut.

Yea its good material to work with. So an old timer recommended .025/.004 doc @ 400 rpm (~260 SFM I believe). That seems way too fast to me. I tried it and it did cut, but did put a lot of pressure on the tool. I tried .017/.002 @ 150 and the vibration seemed to be worse toward the bottom of the thread, nearing the end of the cycle.
 
A 4UN on 2.5" diameter over 28" (presumably) unsupported other than chuck and tailstock?

That's really pushing it, to the point that vibration is guaranteed, not avoided.

If you really have to screwcut it in the lathe, generated form with (much) smaller cutting edges is the get out of jail free card for this. That's not so easy though if you don't have cam that supports it, but it can be trig'd out and put in a spreadsheet for each pass...

Of course this will heavily impact your cycle time, so the quantity you have to do and the time allocated will determine if this is a viable solution.

Yes, good running chuck with a tailstock is my support. Center is running dead nuts thankfully, even out that far. You suggestion, while appreciated, seems a bit out of my wheelhouse though.

We can't make suggestions on speeds, feeds or tell you if you need to decrease your d.o.c. until you tell us what you're currently running it at.
1141 is a nice material to cut.

From a coworker suggestion, I started with .025/.004 ddoc, at 400 rpm (~260 sfm, I believe). It ran, but put a lot of pressure on the tool. I don't think it will work for the duration of the job. (30 pcs. to run)

I next tried .017/.002 ddoc, at 400 rpm and the vibration appeared toward the bottom of the thread, slowed the rpm down near the end of the cycle seemed to help. Doesn't seem like a stable way to run the job though.
 
Yes, good running chuck with a tailstock is my support. Center is running dead nuts thankfully, even out that far. You suggestion, while appreciated, seems a bit out of my wheelhouse though.



From a coworker suggestion, I started with .025/.004 ddoc, at 400 rpm (~260 sfm, I believe). It ran, but put a lot of pressure on the tool. I don't think it will work for the duration of the job. (30 pcs. to run)

I next tried .017/.002 ddoc, at 400 rpm and the vibration appeared toward the bottom of the thread, slowed the rpm down near the end of the cycle seemed to help. Doesn't seem like a stable way to run the job though.

That sfpm is way too slow. You should at least double it. D.O.C. seems fine.
Are you feeding straight in with the cut or on a 60 deg angle?
Can your control alternate the infeed from left flank to right flank?

Unfortunately that's a long hangout without supporting the middle.
You could try to support the center by holding something like a rubber mallet under the middle as the tool passes by, BUT at your own risk because that's not the safest thing in the world to do.

The first thing I would try is to double if not triple the SFPM and decrease your depth of cut. Small/fast passes might just help.
But if you have existing chatter and vibration.... it will be damn near impossible to stop it.
 
Unfortunately, that's a long hangout without supporting the middle.
Simple job running with a tail center.

but with a 4 TPI you are looking at a .250 depth of cut on one side when near done...or going straight in .250 on both sides.

.250 x .010 can be a lot for turning a long part.

One could take perhaps .50 (or .100) depth of cut and run the thread near done.. then take another .050 depth near done.

so the full .250 would only be done at the final finish.

your thread flat would be about .045 so getting/eyeball near that would be cutting close.

re: 1 / 4 =.250. at any speed or feed that is a lot.

This is how I would do it on a manual lathe not big enough for the part.
 
That sfpm is way too slow. You should at least double it. D.O.C. seems fine.
Are you feeding straight in with the cut or on a 60 deg angle?
Can your control alternate the infeed from left flank to right flank?

I cannot control the infeed, though I think Hurcos thread with alternated infeed. It feeds in on a 60°

Unfortunately that's a long hangout without supporting the middle.
You could try to support the center by holding something like a rubber mallet under the middle as the tool passes by, BUT at your own risk because that's not the safest thing in the world to do.

Its a pretty brand new machine and they have it nerfed pretty good. I can't open the door during cycle time without disabling multiple sensors. Which I'd rather not do if I can help it.

The first thing I would try is to double if not triple the SFPM and decrease your depth of cut. Small/fast passes might just help.
But if you have existing chatter and vibration.... it will be damn near impossible to stop it.

That fast you think? Idk, I'm used to slower threading with larger TPIs, doubling the sfm would put me at ~800rpm. Maybe I'm overthinking it
 
That fast you think? Idk, I'm used to slower threading with larger TPIs, doubling the sfm would put me at ~800rpm. Maybe I'm overthinking it

RPM's don't matter (unless the part isn't balanced or in a stable setup) . It's Surface Speed that matters.
If you're going too slow you will be tearing the material off instead of cutting it. Tearing it off will create more tool pressure and also create more vibration.

With long parts, sometimes you have to do the unthinkable and go against all logic. I used to run a cnc lathe that was 120" between centers and there were times when I had to cut an od much faster than I typically would to get rid of vibration.
Long part turning is a different animal at times.
 
RPM's don't matter (unless the part isn't balanced or in a stable setup) . It's Surface Speed that matters.
If you're going too slow you will be tearing the material off instead of cutting it. Tearing it off will create more tool pressure and also create more vibration.

With long parts, sometimes you have to do the unthinkable and go against all logic. I used to run a cnc lathe that was 120" between centers and there were times when I had to cut an od much faster than I typically would to get rid of vibration.
Long part turning is a different animal at times.

Yea, it does make some sense. I'll stick with .017/.002 ddoc, maybe less and up the sfm and go from there. Thanks for suggestions.
 
QT Mtndew: With long parts, sometimes you have to do the unthinkable and go against all logic.

like making a part with a to be cut-off stub at the far end to run in a steady.

I have added side cutting edge clearance, along with back clearance on tool bits..yes on manual lathes.
(I have no experience with CNC lathes.)

Op's insert looks good..I hope it is fingernail shaving sharp.
 
With long parts, sometimes you have to do the unthinkable and go against all logic. I used to run a cnc lathe that was 120" between centers and there were times when I had to cut an od much faster than I typically would to get rid of vibration.
Long part turning is a different animal at times.

My long part story if anybody cares, it wasn't a thread, but it was 321.. and 321 just blows.
Its like 304 alloyed with Ti.. Because it is 304 alloyed with Ti.

1.125 stock. I think the part was 32 inches long, and 28 of it had to come down to .750..

I fought with that sumna bitch, And I was only running half at a time.. Tolerance was wide
open. So I was cutting about 14 inches of 18 sticking out. Tail stock of course..

Had plenty of extra material, and was fed up with it. I was at some god awful huge amount of run
time, and it still wasn't working right... So I took a huge swing from the conservative side
to the stupid side..

Cranked up the surface speed. I'd guess around 400. 2 passes.. Almost .100 each, no finish, and
the faster I fed it.. The better it did. I ended up at I think .014" a rev, just shy of a .100
depth.. Not too bad for a DNMG 432. A couple of minutes instead of a substantial portion of
an hour just dinking with it. The insert had to be changed/rotated every run, but.. Whatever..
I saved about 15 hours, but I ate up a box of inserts.

Sometimes you just have to take a wild swing.. See what happens, it doesn't always work,
actually it usually doesn't work..

--------------

Thought on this one. I think I would run whatever your running now.. Leave the PD a little big.

Then come back in and run 2 separate cycles. Just by changing the start position. A thou or two
z plus, a thou or 2 z minus. Single pass, same depth, maybe a little less.. Take out just the
left and then just the right. Halve your tool pressure and hopefully put it at a point that its
not bouncing around like a meth head that wants to steal your scrap.

The tolerance of the root of a 4 pitch lands in the "who cares" territory. As long as it doesn't look
bad.. who cares.

Edit: thinking about this. Maybe.. Maybe.. having the tool tip on the finish passes buried
a few thou might make things better.. Maybe.
 
Keep in mind that if you have already started a thread on a part, and intend to re-run it, you CANNOT alter the RPM or starting point without wiping out the thread. As soon as you start the next virgin part you can change RPM's, but then you commit to that RPM until the part is done.

This only applies to CNC, not manual.
 
Keep in mind that if you have already started a thread on a part, and intend to re-run it, you CANNOT alter the RPM or starting point without wiping out the thread. As soon as you start the next virgin part you can change RPM's, but then you commit to that RPM until the part is done.

This only applies to CNC, not manual.

And exactly how did you learn this lesson??

Was it the same way I learned it.. At the school of Hard Knocks.
 
That sfpm is way too slow. You should at least double it. D.O.C. seems fine.
Are you feeding straight in with the cut or on a 60 deg angle?
Can your control alternate the infeed from left flank to right flank?

Unfortunately that's a long hangout without supporting the middle.
You could try to support the center by holding something like a rubber mallet under the middle as the tool passes by, BUT at your own risk because that's not the safest thing in the world to do.

I use the rubber mallet trick, but I never suggest that anyone else do it.

If you can use alternating infeed, do it! It will definitely help.
Can you alter/alter your pitch diameter in the middle of your thread, where I am assuming it pushes away?
 
Keep in mind that if you have already started a thread on a part, and intend to re-run it, you CANNOT alter the RPM or starting point without wiping out the thread. As soon as you start the next virgin part you can change RPM's, but then you commit to that RPM until the part is done.

This only applies to CNC, not manual.

Actuall, on the Hurcos, you can change rpm and run again. You can even manually alter it with the override during the cycle and the machine compensates. I didn't think you could, until I was forced to try lol. I don't go nuts with it, but the last part I ran, manually dialing back the rpm toward the end of the cycle helped and the thread looked good.

I use the rubber mallet trick, but I never suggest that anyone else do it.

If you can use alternating infeed, do it! It will definitely help.
Can you alter/alter your pitch diameter in the middle of your thread, where I am assuming it pushes away?

I can't get to the part while the cycle is running due to the door interlocks, else I would totally go for the mallet. You can't alter the PD during the cycle, any changes made to the program while its running go into effect after the cycle finishes.
 








 
Back
Top