Turning 2 degree taper starting at .038 dia on HAAS ST 20 material 316SS

I'm trying to turn a 2 degree taper with a starting OD of .038 and the taper is .375 long. I'm using a custom spring loaded tailstock center (using just the tailstock would bend the part as the diameter got smaller from the tailstock pressure which can't operate below 100psi). I'm currently using a vnmg profile tool with a .015 tool nose radius.
any suggestion on how I can accomplish this would very helpful.
Thanks,
Scott

A Single pass will probably be the best bet.

What have you tried so far?

R

I've tried roughing at .01 then with a .005 finish pass at .0008 ipr. I have not tried single pass yet. I'm also waiting for an 00 center drill. right now I have a .03 center hole which I think is also not helping my cause. I will try a single pass on the taper and let you know how it worked.
thanks for the input!!!

Use a positive insert with a fine chip breaker for as little tool pressure I guess

Sendt fra min EML-L29 med Tapatalk

Try roughing out just a small portion of the taper, finishing that; rough out a little more, finish that; rough out the rest and finish that. On some flimsy lathe jobs that's about all you can do.

Either that or rough and finish the tip then make a shop-made female center to go over it for support.

Minimal tool radius (.008 or less), being exactly on center and having a positive cutting action will be key.

Are you cutting toward or away from the tailstock?

What is the length of the taper? What diameter do you end at?

Stiffness of the setup, sharp cutting edge, minimal TNR, and depending on stock diameter, try roughing down to a ~.13 start diameter, then a finish pass to remove the rest in one pass.

If your stock is small to begin with, you need to hold it with a tight collet or reducing bushing in a chuck, with a good pressure to keep the stock from wiggling. Too much stickout will make life miserable.

BTW, I don't see a need for any tailstock support unless you have to turn additional features along the length.

I agree with Rob on one pass. Adjust the program to get the results you want.
Runout needs to be dead on otherwise at that angle will give you a funky washout.

I'll also add my favor to single pass..

What is the starting diameter of the stock? There are times when you actually end up
money and time and aggravation ahead by buying larger stock than the part actually
fits into..

Are there any other features beyond the taper? How long is the stick out?

One pass and done is the way to deal with *some* things, and this sounds like
one of those things.. Shouldn't need a fancy center, shouldn't need
a fancy center drill. Up-size the material if its sticking out a mile, and
one shot and done.

This is one of those learning experiences where conventional machining knowledge
loses.

Also.. What are you using for an insert? This is one of those cases where you
are going to be surface speed limited, so a conventional insert is going to
screw you.. Uncoated, ground, high up-sharp insert designed for aluminum
will probably do you pretty well. Kind of like a super sharp piece of HSS,
but you don't have to grind it, and its got a lot larger range of surface speed
it can deal with.

I'm starting with .25 dia 304ss its a 2 degree taper with a small end of .037 dia for .375" long finishing at approx. .064 dia I've tried turn in both directions so far. I'm wait for a new insert which is .004 TNR.
Thanks for all the input!!!!

orionsgn said:

I'm starting with .25 dia 304ss its a 2 degree taper with a small end of .037 dia for .375" long finishing at approx. .064 dia I've tried turn in both directions so far. I'm wait for a new insert which is .004 TNR.
Thanks for all the input!!!!

Click to expand...

It really is a Swiss part.

Hi Orionsgn:
All good posts here; I'll just add a few tidbits from my own experience ( make lots of tiny stuff).

I will often take the insert and nip off the whole tool nose radius, then diamond hone a new one that's only 0.001" to 0.002" radius...just enough so you know it's there when you look at it under a microscope.

The second thing is to get it dead nuts on center or maybe 0.0005" below for external turning on small diameters but not more.
No that's not a missed zero...half a thou below MAXIMUM is what I go for, and I drop gauge each tool to be sure I get it there.

Now... I have a gang chucker instead of a turret machine and I run a lot of tools in parallel shank ER collet chucks so I can just rotate the collet chuck body to get it dead nuts and drop gauge off the table.
You will have to find another way...maybe a LH boring bar in a sleeve so you can do the same to get it as close to perfect as possible.

I typically do these things in several stages as Jobshopper TN describes in post # 5, but I program each segment of my finish pass with a radiused lead in and a radiused lead out and I leave VERY LITTLE for my finishing pass...maybe 0.001" per side using a very sharp insert with positive rake and the tip ground off on a super fine diamond wheel as described above.
My chips are like fine steel wool and no I don't try to chip break.

I also run cutting oil in my machine or just squirt on some Rapidtap if I don't want to slime the whole machine for one or two parts.
I typically start with oversize stock as BobW recommends in Post # 9 so it's nice and stiff.

If I have a bunch to do. I set up a separate finishing tool so I can preserve it, and my finishing passes have (naturally) a very slow feedrate so my miniscule corner radius doesn't end up cutting a thread instead of a finish pass.
I might go 6000 RPM and 0.0002" IPR to 0.0003" IPR.

Yes it all sounds terribly wrong and it'll rub and not cut and etc etc, but for weeny tiny skinny stuff it seems to work best for me, especially if I need to hit a good finish in 304 SS and don't get to abrasive polish in order to wipe out toolmarks.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

2outof3 said:

It really is a Swiss part.

Click to expand...

I'd have made 10K of them since the time this post was made. But, y'know, he's gotta run what he brung. Hopefully the good advice in this thread will help him out.

TeachMePlease said:

I'd have made 10K of them since the time this post was made. But, y'know, he's gotta run what he brung. Hopefully the good advice in this thread will help him out.

Click to expand...

I sure as shit would have at least one done, so I could wake up the hamsters, and report back here how it went.

R

litlerob1 said:

I sure as shit would have at least one done, so I could wake up the hamsters, and report back here how it went.

R

Click to expand...

It's possible he, ya know, does other things than just this one part.... just a WAG though.

Mike1974 said:

It's possible he, ya know, does other things than just this one part.... just a WAG though.

Click to expand...

Wives And Girlfriends have nothing to do with whether the part got off the Machine.

It is a pet-peev when people ask then don't get back to us. TMP could've made 10k, worked up a batch AND responded. Back to the hamsters jogging that wheel behind the monitor of the computer?

R

1.
A suggestion .. perhaps ...
a shop made female dead center made somewhat oversize, with a slot cut in it, in phosphor bronze/sintered bronze/miracle plastic/similar might allow you to rough oversize, and then use the center to support the part.

Then finish-cut through the slot, one pass.

Kind of like a custom jaw/pie jaw/soft jaw but in a lathe.
Like a fixed steady but as a TS and with custom shape to the roughed-in outline.
Should work, maybe, as the guide bushing in swiss-type lathes.

---
Also..
Might be ways to reduce pressure of the TS center, like a support nub near HS end that the custom center leans against.
Or belleville springs.
Or Tapers/nubs at one end resting on the ts center that get parted off at the end.
Or float the part in an internal reamed chamber, tensioned via spings/bellevilles, from HS to the TS.
-- Rest TS against the fixture body and not the part.

Qty, value, volume affects what makes sense.
Bar-fed, volume, everything is critical, like always.
---

2.
Looking at it like old-school roller-box threading tools to finish with might also work.
For Finishing, mostly, perhaps.

E.g.
A closed form tool with interrupted cuts, think reamer with some flutes interrupted internally in a helical pattern.
Like a roughing end mill, kind of.
Maybe some holes reamed in to let the chips out from the tool.

2-3-4 tools mounted in one tool-holder.
Use like a gang-tool lathe, but only one turret tool used, indexing in x and not turret, since the parts are small.

Could make the individual form-tools in 2 halves, finally pressed in to a holder.
Even hand-work for cutting the flutes should work.

So without doing a toolchange, just pull out in z, index in x, do next form-tool cycle.
Could be only a few seconds tool-tool, and only a few seconds in the op.

Justing making suggestions, and most above I have seen used somewhere, to some extent.

Many years ago, early in my cnc career, I made a batch of jet needles for a vintage carb on a simple cnc centre lathe.

VBMT cermet insert, .2mm rad, single pass to turn profile, cut the threads, part off.

It worked flawlessly and I have reused the technique many times since.

So, a long winded way of saying "+1 for the single pass".

I don't think it will ever work well with a VNMG tho, unless you can find a single sided high positive type.

I see no reason for a center, nor a Swiss with what info we have been given here so far.

I too would recommend a rough down to 1/8 or so, and maybe even taper that up a bit too?
Then one pass to finish with very low feedrate.

I just kan't imagine trying to stuff a center in a .038 shaft!


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

Think Snow Eh!
Ox

No center, DCGT 2(1.5)05, the ones for Al... done thousands of skinny little parts in 316 with those and good tool life. Low feed, I don't try to break a chip on small stuff. Good fairly rich coolant or oil.
I'm assuming you're holding with a collet, 5C or such, stick out minimum.
It could take a bit of tweaking to get the taper just right though, and stuff that small isn't super fun to inspect. Depends how "bang on" its gotta be.