Need Help!- Deep boring on a horizontal lathe

[freeportcncdude]

I am boring a 4.500/4.503 hole diameter from an approximately 4.02 diameter drilled hole. The hole depth is nearly twenty five inches deep. The material is 4140/4142 hardened 28 to 32 rockwell. I am using a 3 inch diameter Kennametal tunable boring bar with a KM63 head for a Kennametal CCMT 432LF KCP25 insert to rough out the bore. I am trying to leave .010 to .020 to finish. I am finishing with a 2.5" Sandvik Silent Tools boring bar with a Sandvik DNMG 431-PF 5015 insert. I am having to rapid the finish boring bar to the bottom and feed out of the bore to keep from having a big ball of chips in front of the boring bar that would get compacted in the bottom of the bore. The ball of chips causes problems with the finish in the bottom of the bore. I am running 600 SFM at .012/rev feed for the rough process. I am running 600 SFM at .009/rev feed on the finish process. The rought boring bar is hanging out 31.625 inches. The finish boring bar is hanging out 25 inches. I need to hold a somewhat decent finish because I am burnishing with a Cogsdill roller burnisher to a 20 finish. This is all being done on a Cincinatti Milacron 18U turning center with a 100 inch bed.

I am looking for better ways to do what I am doing to make this part simpler to run. I have no control of the process and would like to get to a more stable controlled process. I am open to looking at suggestions.

[Delw]

Sandvik made a really cool chip breaking insert years ago, I cant remember the number as its been 8 years since I used them.
they had a big bump just after the chipbreaker( I mean a tall radical angled one.
it would break a chip with as little as a .004 finish pass on 9310 gear steel in the same RC. I think they were avail in .015r and .008 rad. we used to do some bottle bores and had that same problem. Granted not the size of part you have not even close but it was the same problem.
our inserts were ccmt style. they were a tad expenisve but they were well worth it, The sales guy told me about them and I laughed at him for about a month then told him to prove it. when working with the guy they didnt work per spec. however if we increased the feed rate a tad they worked great.
it was one of those cases were the sales guy was right for a change, and he got to say I told you so lol

I Think cermet also had something similar as well however you had to run a very high surface footage.

[Brakeman Bob]

Is this likely to be a repeating job and if so, how much are you prepared to spend? Have a look at a gundrill for finishing the bore and also think about a steady or work support as the overhang will make the whole system of tool & workpiece unstable and once you get resonance going you're buggered. If a steady is out of the question, consider getting someone with MetalMax to come and analyse your set up with a 'tap hammer' as a small change in speed & feed may bring the system into a zone more stable than where you are now (and there is as much likelihood the spindle speed goes up as it goes down).

Doing a job similar to this many years agoe (8" bore by 37" dp) I saw a setter start wrapping rubber rope (like a bungee but far longer) around the workpiece in an effort to damp out the vibration that was the cause of the poor finise we were getting. Odd I know, but it helped.

[skucku99]

cool i work in the company that make this tools teeness (sandvik)

10xD is the max.
is 0.02 the radial cut ?

jan

[freeportcncdude]

In reply to Brakeman Bob I am not sure if it is going to repeat or how often it will repeat. This is a new concept for the company I work for. Since having bought the 100" bed lathe we are trying to do more of our own deep hole product machining in house. The company would normally send the work out to someone else to do. Fortunately I have not had any problems with chatter despite the boring bar overhang. My biggest problem is getting the rough boring bar to repeat a consistant amount of stock for finishing as well as chip control. At the present time with the insert I am using to rough bore with and the approximate .100" to .125" depth of cut and the speeds and feeds we are running I am getting rather good chip control. I could use a little better chip evacuation yet though. I am running a somewhat moderate pressure and I believe somewhat moderate coolant volume for chip evacuation.

In response to skucku99, yes .020" would be a radial cut.

[skucku99]

well if u ask me the kenna bar is not so good as the sandvik bar

whene we use the long bar its wery importent that the cuts are same because it will bend of therefore it is normal to use 2 fine cut....

u can try smaler cuts too get smaller chips..? is it a ds97 bar ?

[freeportcncdude]

Smaller cuts like .065" deep have proven not to work. Smaller cuts cause chip control problems. My only success with chip control in the rough boring operation has been to take the .100" to .125" depth of cut. I am unfamiliar with a ds97 bar. The Kennametal bar is a D48TTB45KM63 and the Sandvick bar is a A570-3C D40 33-60.

[skucku99]

yes thats ds 97 (dempe system 1997 ) some thing like anti vibrant system 97.

u are having problem with rough boring operation.

so the fine cuts are ok ?

here we stop the bar and flood it with coolant too flush out the chipps.

and then start upp again. important to stop cause the centrifugal force make it harder too flush out chips ..

jan

[freeportcncdude]

Fine or finish cutting is working alright. I need the rough boring bar to leave a consistant amount of stock to finish. It seems like the deeper the rough boring bar gets the more it is pushing off causing the hole to be up to .100" smaller at the bottom of the hole. I will try a program stop(M00) between the two rough boring passes and flush out the chips to see if that might help the hole size at the bottom of the hole. Thanks for the suggestion skucku99.

[LatheMaster]

What a nightmare . I have never tried running a tool that size , that deep . I am surprised chatter isn't an issue . I can say I have tried to run a finish tool backwards for the chip issue . I found it really caused the tool to deflect and I was always having to take a spring pass . Bringing on to size became a guessing game trying to hold +/-.001 . I ended up doing the part in sections . Each finish section I bring the tool in on a taper to meet the prior cut . Maybe with the rougher you can do the same . I run the hard stuff at 425 SFM .
And .015-.018 feed to get a good chipbreak . If I am sturdy enough I will go even higher but your hangin out too far for that .

Ever thought of send them out to be honed to bring them on to size ?

[skucku99]

the tool u are using is good for 0,02 mm but u need too do 2 fine cut...

because it will bend of realy much...

i use these tools every day and i make theme as well.

try programing it too flush, all in, slow rotation and feed it out slow 1/2 in peer rev.

but u must have chipp controll no long chips

jan

[Andre' B]

I do not have much to do with lathes but if I were doing that on a mill I would be looking a something like Kaiser twin bore tools.
http://big-tooling.com/frm.htm?news/mms-reduce21-9.htm
Better example.
http://www.kaiserprecisiontooling.co...e-dbl-head.htm