[dingo0722]

I am using a 0.157 wide parting insert and it seem that every combination of speed and feed I have been using gives me a bad finish. I am starting out a 2.3" in OD down to 0.4". When I crank the RPM to 2000 I get an improved finish when using a constant feed of 0.002ipr but I still get some chatter. Any help here would be great

[fizzissist]

1st rule of chatter.... slow down the rpm, or increase the feed.

But that presumes you're cutting as close to the chuck/collet as possible, and the tool is clamped as close as possible into the holder. It's a rigidity thing. And, the tool is on center to .001/.002 above center.

My first take on this would be to do a little of both here... I think you're in the fine-tuning regime.

[txcncman]

Are you getting good chip breakage and evacuation? I have seen before that chips will be too large and can bind in the cut and cause problems. Sometimes switching to a peck can help break the chips and allow them time to exit the cut. One peck per revolution works well but takes more time. That is if you are feeding at 0.002 make your peck at 0.002 also. Also tool tip not on center line will cause problems.

[Shane1234]

i would go with a g96 s450 and keep your feed at .002 ipr. i hope your not using a blade, i try not to use the blade if i can get away with using my other parting tools. blades are really good for long reach, but thats about it, in my experiences......

[dingo0722]

So I am setup for production of the part now but I cannot get the parting tool to exceed G96S97 with a F0.002

I have now set up the parting operation to go Z-0.005 more then follow up with a finishing parting operation at the correct z location. I run that at G96S150 F.002 and get an acceptable fish.

I have tried adjusting the turret angle in both the + and - degree rotation with no success. Current run time on this very simple part is 4 min due to the parting tool operation; it should be more like 1.25 min

The stock is 2.375dia 303SS. OD is turned down to 2.3 and a 1/2" center hole is drilled

I am using a Tungaloy parting tool and their angled insert

I have bored the jaw to 2.37 and put in a slight tapering angle going outward as you go more - in Z

The stock is a 4 foot long bar supported with a spindle liner that is tight in both the spindle and the bar

Not sure what is going on here. Any help would be great

[txcncman]

Well, there ya go. Tungaloy. 0.157 wide. Switch to an Iscar tool, 3mm wide, and your problems will melt away magically.

[Delw]

you have a few problems, one with a blade tool that small your angle inserts arent worth it. use a flat insert, Ive tried the angled inserts from iscar and sandvik and unless its brass or alum I had very little luck I waste more inserts than normal.

for 303 stainless and a quality insert go with sf of 450 or lower, I generally go on that size when parting off 300 and inserts last forever.

those sf are for decent part lengths, if you have a long part then you need to slow way down.

Dont peck with a angled insert .

I noticed you used a spindle linner that is tight, so you know what your doing, I also noticed you put an angle in your jaws, unless your running runns in 3" of length or more its not needed even at 2" length anything over .001 is too much, this could also hurt you when using angled inserts as they will pull/push stock when cutting.

Angled inserts are nice but in most applications they are not justified and will cost you more in time and insert replacement than its worth.

if your trying to make it so you dont have a secondary operation(chamfer on I.d. Back side) grab a chunk of carbide or a thread cutter and go through the I.D. and make a small chamfer in the back. small tpg boring bar works well also, then part off and your burr free. with just some minor lapping on a pcs of wet dry paper for the back side.


Delw

[dingo0722]

Thanks for the feedback. Well after getting off the phone with Tungeloy, it appears they produced some out of spec tool holders that puts the cutting tool off center. They are overnighting me one now.

They claim that I should be able to run G96S500 with a F.004 to.005 with excellent results in 303.

we shall see tomorrow. I hope this is the case and with the increased speed I can make up for a lost day today

[Shane1234]

that sounds better. dunno why you were running soooo slow....... i run my sandviks at 450 sfm in ss303 & 304 all day!

[underthetire]

I agree, that insert is pretty wide. I love the iscar stuff as well, that with high pressure coolant through the insert makes a huge difference.

[txcncman]

He slowed the RPM down trying to compensate for improper cutting. Even though he checked the tool tip for center line, he did not notice that the rake angle of the insert was such that there was no relief clearance on the tool. Since there was no relief, the face of the tool was riding on the material, basically extruding its way through the cut.

Well, that is my pseudo-scientific explanation any way.

[ctate2000]

Is your turret properly aligned?

[Delw]

that sounds better. dunno why you were running soooo slow....... i run my sandviks at 450 sfm in ss303 & 304 all day!

Shane
I run 303 slower than 304 with sandvik tools, its more of a personal preference for me. the reason is 303 is really abrasive and tends to wear the tip of the insert down faster than 304 does, yes 304 is tougher to cut but it runs smoother than 303 especially on cut off and facing tools.

one machine (omni turn )we run 303 in runs only oil and that machine we can run a cut off blade for 1 year(micro 100 cut off blades) on 303 and not worry about wearing it out. it runs every day on 3/16 dia to 5/8 dia 303 stock.
it runs a .025-.050 chamfer depending on part dia. and cut off .
used to cut tons of 303 in 2" and up( in bigger lathes) and I always cut down the SF on 303 vs 304 for the same reason.

Delw

[Shane1234]

Shane
I run 303 slower than 304 with sandvik tools, its more of a personal preference for me. the reason is 303 is really abrasive and tends to wear the tip of the insert down faster than 304 does, yes 304 is tougher to cut but it runs smoother than 303 especially on cut off and facing tools.

one machine (omni turn )we run 303 in runs only oil and that machine we can run a cut off blade for 1 year(micro 100 cut off blades) on 303 and not worry about wearing it out. it runs every day on 3/16 dia to 5/8 dia 303 stock.
it runs a .025-.050 chamfer depending on part dia. and cut off .
used to cut tons of 303 in 2" and up( in bigger lathes) and I always cut down the SF on 303 vs 304 for the same reason.

Delw

i have noticed that with my finish turning, however 99.99% of the time we are up against a wall with time, so we tend to sacrifice longevity for over-all time. sfm of 450 for my rougher & parting, sfm 650 for my finishing and shallow grooving with parting blade, and usually baby threading & normal grooving tools. i still havent found anything that will keep up with the 1125 grade sandvik in 303 & 304, however the seco makes a wnmg rougher that comes close.

[Delw]

shane I think i know what secos wnmg your talking about those are fantastic inserts, they last longer then the sanviks for 9310 gear steel and 1045 too. I use them for rough cause I get alot more parts per inserts.
I got like 1 box left.
BTW were do you get the seco the place I used to get them locally closed many years ago.and I havent looked for a new place yet

[Shane1234]

shane I think i know what secos wnmg your talking about those are fantastic inserts, they last longer then the sanviks for 9310 gear steel and 1045 too. I use them for rough cause I get alot more parts per inserts.
I got like 1 box left.
BTW were do you get the seco the place I used to get them locally closed many years ago.and I havent looked for a new place yet

we get seco from deco tool
Home

the main problem we have with inserts is jumping from sqaure shaft to round bar to hex, etc, in stainless steel. the 1125 grade sandviks take the abuse of the interrupted cut and keeps on chugging.

we do use the cheaper mitsubishi inserts when we machine 1018, 1045, and 4140, as those seem to handle it just fine.

any insert works for delryn, but we have some sharp edge prep non coated inserts for uhmw to help from stringing up.

[Delw]

for a interupted cut wnmg 432 I use the valenite wnmg-432-lm-sv325
have very good life in in hex and casting along with heavy hot roll scaling and other interupted cuts.

Thanks for the link
Delw