Rough Boring Help

Ok. So Ive been programming/machining for around 8 years now but until a year or 2 ago, been mainly running mills. We have an integrex (millturn) in the shop that the two older guys HATE programming because we do it EIA/ISO by hand. So I took it on and have been working with it for a while now. Its been a learning curve on the turning side, mainly learning how to turn at much much higher surface footage. I had only really run manual lathes before the integrex and never really ran fast. Ive got OD turning down pat and can get fantastic results. But when it comes to boring in steels (we do a LOT of 4130/4340 heat treated to 150-180kpsi 35-42rc roughly) i cant get bars to not chatter. Ever.
Currently I am running a driveshaft end (splined on 2.5" end and then it tapers up to a 4.118 journal with a 3.8" ID) made from a 4340 forging heat treated to 38-42rc. I am running the first setup. I have premachined a journal on the small end and am clamping in 3" machined steel soft jaws. The part is 8" overall in length roughly. So the big "bell end" is hanging out. Unfortunately, the spindle thru bore is only 2" so i am unable to fit part into spindle to shorten the stickout. I am drilling 1.5" dia with a carb spade drill about 4" deep. Then i am proceeding to rough out the id with a 1.25" A20-MCLNR boring bar using a CNMG431 insert. 1.25" is the largest bar the lower turret will fit. (On a side note, ive tried using some large insert drills to rough out the part, but given the length of the drill and the part reach, they instantly chatter and break inserts. Ive tried milling and plunge milling but they also destroyed inserts...) So i resorted to boring. Ive got deadlines to meet.

My question is in regards to general speeds and feeds when rough boring alloy steels that have been heat treated. Even in parts not hanging way out of the chuck i always get chatter in steel. Regardless of bar size. Carbide bars only run quiet at slow speeds. Ive also bought split sleeve adapters for the tool blocks to try and damp the vibration but they only help minimally. So i am roughing this steel with my cnmg431 at 200sfm (bar is extended 4.5" from tool block, no split sleeve as tool block is 1.25 ID) .05" radial doc, .01 ipr. The chatter is higher pitch and constant, but i can get about 4 parts before insert starts to break down. I noticed on my finishing bar (also a 1.25" bar but uses a vnmg or vpgr top notch insert) that it would chatter until i really crank up the sfm. At 500sfm, it runs like a wet dream, even with the knurled finish from the roughing bar. Babys bottom finish that shines. And Im scratching my head.

Do I need to crank up the sfm on my roughing bar? Does that increase tangential force and load the bar? Do i need a heavier doc? Higher feed? Ive tried up to .015ipr at .05 and it only worsens the chatter. Ibe tried increasing the speed by maybe 20-40% on the control but it worsens the noise. What do you experts do to quiet boring bars? Unfortunately this is a semi long run and i cant run 70sfm to quiet it. Aint nobody got time for dat! Its been recommended to us by a fellow shop that tunable bars are the way to go but the smallest i can find is 1.5 and quite expensive. Want to see if i can optimize this steel bar first. Should i run higher sfm with lighter doc and heavier feed?

Thanks in advance for any pointers. If i forgot to add any info, let me know and Ill correct.

I'd definitely take a deeper cut. You aren't even burying the Radius of the insert. Boring is a bit of voodoo sometimes.

R

I use a WNMG (trigonal) insert boring bar for most of our boring ops.

I don't have an Integrex, but on a normal lathe I'd never run a cnmg at less than .015" feed. And your depth of cut, yikes. 3/16" (.1875) on a side is about what I shoot for when roughing. And why 431 ? Too sharp a corner, imo.

For speed, 400 sfm is my "basic steel starting point" .... up or down from there depending on how it's working.

vnmg for finishing ? Ick. I despise those flimsy feeble things.

If an Integrex is flimsy I guess you can't run those numbers, but .... inch anda quarter boring bar is okay for sturdy, not like a flimsy little 1/2" thing. If the bore is really deep you may need to go with something built for that - solid carbide ($$$$) or one of the de-vibrator bars. But to me, at this point you aren't taking a cut, you're trying to scare it off. That leads to chatter.

If you are going to run light cuts, get away from negative rake inserts. They like to be loaded. Maybe try a Sandvik knux ? I am a big fan of those for jobs that need finesse. And the devibrator bars do work, but don't pay their outrageous prices, make your own. Bore the boring bar out and fill it with lead shot. Put a threaded bolt in the end so you can adjust the internal damping of the bar. Carbide balls work also, maybe even better.

Or buy a real lathe where you can bury the part in the spindle

theperfessor said:

I use a WNMG (trigonal) insert boring bar for most of our boring ops.

Click to expand...

You use WNMG when you're fighting chatter in a Bore?

The Heeb is about right. Turning is hard and fast, treat it that way.

R

Do what EG said above and use a positive insert like a CCMT or WCMT 32.52. They usually have lower cutting forces than "X"NMG inserts. Think of it as using a knife or a cold chisel to cut wood. The knife will take less effort, because it whittles away at it instead of bulldozing it off. However the cold chisel will have a stronger edge and will resist breakage.

All the above and watch your overhang- 4.5 inches out on a 1.25 bar is between 3x and 4x overhang and that's just about where things go upside down. Always minimize your overhang- if you are using coolant thru bars, get the toolholder or turret face right up to the part as much as possible or leave just enough room to get coolant in there. You can get positive rake CNMG inserts, but get some .032 R inserts.

litlerob1 said:

You use WNMG when you're fighting chatter in a Bore?

Click to expand...

Sure do. We use a 1" bar to bore almost 5" deep in 8620. We drill out a solid 2" bar to 1-7/32" and then bore from either end to make a 1.375 straight bore on one end and a 1.5" (at the opening) tapered bore on the other. We do not run these out of a tool post, we have them rigidly mounted to the cross slide of our TL1 in a custom tool holder setup we made (gang tooling).

Can't find photo right now but I'll keep looking.

OK here is photo of bar stubbed up for different job and mounted to our gang tool setup. Much more rigid than working out of tool post.

Yep, that works. When I read your first post a mental image of something else popped up. Too many nomenclatures.

R