[BTC 111]

Hello everyone,
I'm having an issue with finish when turning small stainless pins.
For an industrial part we would be fine, but this part is a jewelry piece and it needs to look better coming
off the machine.
The part is .140 OD that has to be faced, chamfered, and then the OD turned.
The head of the pin is only .045" long. It just needs to look better. I'm using a CCGT insert with a .004 radius
made by Kennametal now. But I really need to use a 35 deg tool but that is extremly sharp and that will cut when making very light cuts.
The machine is an older Nomura 16KFC but that is holding great tolerance and it's extremely accurate. It has a fixed bushing and will only run 5500 rpm max.
The stainless bar is Ugima 303 .156" diameter.
I'm turning using a .001-.003 depth of cut and a .0004 IPM feedrate.

Any tooling you guys can recommend for something like this?
I've been told that NTK or Mitsubishi is the way to go.
But????

I uploaded an pdf file of the basic pin.

Any help would be great,
Thanks

[ebischoff]

First thing to try before different inserts is a deeper DOC.
Your insert NR is bigger than the DOC you are turning and tool is skipping over the turn.

Try .006" to .008" DOC and follow recommended speeds and feeds for the insert.

Good Luck

[danrudolph]

The stainless bar is Ugima 303 .156" diameter.
I'm turning using a .001-.003 depth of cut and a .0004 IPM feedrate.

This is a swiss machine? So .001-.003 DOC makes no sense, should be one pass, assuming .0004 IPM really is .0004 IPR.

303 is going to look dull and crappy most of the time coming off the machine. 304 or 316 would look awesome without much effort.

Look at NTK's CSV line of inserts, they have no nose radius, I use them on a similar 303 job that looks like yours, but smaller.

[elsanch]

you might want to try a grooving insert....031 wide..use a holder from ISCAR that is used fro grooving/turning...and parting off...maybe try G96 for the angle so the chip load stays the same throughout cut. the angle would look better.

[Benpen]

Dan has it right. It's 303. Cut it in one pass at 3000 rpm and .001 - .0015 ipr of feed. Will cut great and look fine.


Sent from my iPad using Tapatalk - now Free

[micky316]

use a wiper insert and turn at 3000rpm with a federate of .002" per rev or if that's no good try a precitool or applitec grooving insert that will rub as it cuts as well
Mick

[fizzissist]

Browne & Sharpe makes ( or at least made ) a "box tool" that would be ideal for this .

One pass, it takes a large depth of cut easily, and burnishes at the same time. The trick is having the regrinding fixture for it. I don't know if
they're still available,, tool and regrinding fixture,, or if you can get pre-ground carbide tools for it.

I've used them in automatic screw machines for decades and when set properly, they'll hold within tenths and give you an easy 16 finish. Haven't done 303 with 'em, but have done 304 duplex and gotten very nice finishes.

Here's a photo....
Photo of - BOYAR SCHULTZ / BROWN & SHARPE Box Tool

.... Just looked at the drawing... the step suggests a skiving tool.

[DCogswell]

Fizzissist, where in Reno is your company located?