I have a question about using a 1/2 carbide boring bar. I am boring out an ID on a CNC Lathe using 1/2 boring bar, the boring bar is hanging out 3" :( . I am only taking .003 per side and I am getting the wrinkle affect on the wall. I have tried it at numerous feeds and speeds and can't get it to work out just right. The last run I was running at 1000rpm with a feed of .004 and the finish came out great, so I put another part in and got a wrinkle finish so I was back to the drawling board all over. The material is 6061-T6. Any suggestions out there?

Machine1

What style of insert are you using? That is one aspect to play with.

The other one, is to rotate the bar so that it does not have excessive front clearance. The default bar clearance is designed for the minimum bore, and if you are working above that, you should be able to rotate it a bit to reduce the clearance, and improve the top rake angle all in one go.

The way the bar is clamped is also important for damping. I regularly bore with a 1/2 steel bar and 3" overhang without too much trouble. The bar is cradled in a V block holder, and setsrews on top, nothing fancy, but for sure, 6 point support. I also use relatively massive Kloppfer style toolposts on a 19" lathe :D

Originally emailed by Machine1
I am not 100% sure which inserts they are using. We kinda have a select few until monday. Do you have any suggestions. I believe that they are CPMT. What do you think we should go with?

Hi Machine1

Sorry to not get back to you sooner. The nose shape of a CPMT is likely the culprit. The shape of this insert creates too wide of a cutting zone on the front, which increases the pressure requirement, and so the bar floats on top of the work to some extent, and results in chatter.

For best boring performance with a small, overhung bar, you need to go to an insert with a more acute point, like a T shape (60degree) or even more acute. The acute point tends to bring only a very narrow zone in contact, and will cut pretty good. I use a simple T221P insert and bar and have excellent results.

Hope this helps. Sorry if you spent big bucks on that other bar just for this job. Maybe you can return it and exchange it.

Sometimes the solution for chatter is to "really go at it". In other words, get the tool under a good chip. In aluminum, you should be running very fast (to get good chip flow), and at least .01" depth of cut. Take advantage of your insert shape by feeding at about .007" per rev. That is why you are using this insert, to reduce scallop height at an increased feedrate, so do it! :D

The advice worked great on this job and I know that I will be able to apply it to many more like it. I used the T shape insert and up'ed my RPM to 3000 on CSS and fed it at .007". Awesome results! Needed 125 Surface Finish and got a 48 with no wrinkle or chatter.

Thanks:)

Originally posted by HuFlungDung
Take advantage of your insert shape by feeding at about .007" per rev.

Do you guys program in imperial then. Never seen that Before :eek:

Originally posted by M@T
Do you guys program in imperial then. Never seen that Before :eek:

Yeah, most of us do. Well, many of us do. ;) There's lots more companies converting these days, but I don't think we'll see 100% coversion in our lives.

'Rekd teh damn yankees!

I live in England and over here you'll struggle to find a machine shop that programs in Imperial though many places use imperial drawings and measuring equipment especially mics.

I prefer Metric TBH :cool:

Canada is supposed to be metric, too, but you have to go to the States to get metric shafting, and they're still on the inch system!

So this makes it a real mess, about 4 thread systems on the go, and only inch based stock readily available.