Just can't get any sort of good finish boring aluminum on lathe - tips?

[SRT Mike]

I have a project that requires a cylinder of 6061 T651 aluminum 1.1" long, 1.7" OD and 1.35" ID, then at the end of the cylinder the ID goes down to 1.30" for the last 0.120" and for the last 0.020" it goes down to 1.25".

I am trying to make this on my Okuma lathe. I am running the spindle at 1500rpm, I know higher would be better, but it's got a 12" chuck and it already sounds like an airplane about to take off at 1,500 so I don't dare go higher! I am cutting right up against the chuck, the stock only sticks out about 1.5"

Anyway, I start by drilling a 1.00" hole, then I bore at 0.100 depth of cut, 0.002 IPR at the aforementioned 1500rpm. The boring bar is 0.375 dia with a CCMT 21.51 positive rake insert and the bar extends about 2" out of the holder.

I've tried varying the DOC between 0.050 and 0.100 and varying the feed from 0.001IPR to 0.008IPR. The finish is horrendous every time. I've made sure the orientation of the bar is good and the insert is cutting at the correct position, etc. I've tried taking a 5-10 thou clean up pass and it just squeals like a pig during the cut and the finish is as bad as ever (I am using flood coolant aimed pretty well at the insert and not being blocked when cutting)

Now I know it would be ideal if I could run a larger size boring bar, but I have other jobs that require the smaller bar, so I am really hoping I can get this finish issue nailed down so I don't have to buy another boring bar and swap out the tool just for this one part.

Can anyone suggest what I am doing wrong? I may be waaay off on feed and speed, I've just been messing with it after my original calculations for feed and DOC produced a horrible finish.

And by horrible finish, I mean a diamond scalloped pattern that must be a good 15 thou deep. Incidentally, if I run the exact same program in a piece of brass, it is smooth as glass, inside and out.

What should feed and depth of cut be for this setup?

If I am in the ballpark with feed/speed and it's the flexing of the bar and I need a larger one, would a different insert geometry produce a better finish? I do need to get right into the corners with the boring bar because I have shoulders on the ID, but I am open to a different tool setup if it would help and if this problem can't be solved by adjusting my current setup.

[Geof]

Try running lower rpm and faster feed. To avoid chatter when boring small diameter in 6061 I have even gone as low as 600 rpm for 1" ID with 0.005 ipr and .01 doc on the final pass.

Also try tricks like wrapping tape and solder around the boring bar where it does not enter the hole. Wrap a few layers of electricians tape, then wind the solder (the stuff you get in a coil for doing copper pipe) on as tight as possible and cover with a few tight layers of tape. The idea is to try and kill any resonant vibrations in the boring bar.

[N-see]

The first thing I would do is to make sure the tool you have in is actually positive rake when clamped in the tool holder. Make sure the cutting edge is sharp and not chipped or loose in the holder.
I would recomend a cutting speed of... 150 S.F.P.M. / 45 m/min.
Use a soluable oil or RP7 or Linox, but you must use something.
If you are still having trouble with a finish try a HSS groung tip, aluminium loves a very sharp tool for cutting abd not all replaceable tips can be as sharp as a high speed tip.
Try roughing cuts to near finish diameter, then one light finish cut, if chatter lower the revs.
All the best.
N-see

[Mike Stevenson]

What type of insert are you using? Have you checked the center height of the insert? Is the bar held firm in the turret holder? You know, the basics.

[DareBee]

Forget all that. Get a new boring bar.
You need 1 that is largest dia possible to do the job. Best is carbide or heavy metal shank (but not likely needed for this job).
CCMT is not the best designed insert for this job but we use them frequently with good results.
Get a bar that you can buy Aluminum specific inserts for such as a DCGT and the bar can have a 3/4 or 5/8 shank.
I have bored aluminum as deep as 15" with a 1" shank bar on a lathe nowhere near as rigid as yours and the aluminum had 1/16 wall thickness when done. About 350 SFM .02 DOC and .009 IPR - These are really weenie numbers (if you saw what I was doing you would understand) but YOU should be able to go hells bells with the right bar and your setup.

[chrisryn]

Originally Posted by Geof Try running lower rpm and faster feed. To avoid chatter when boring small diameter in 6061 I have even gone as low as 600 rpm for 1" ID with 0.005 ipr and .01 doc on the final pass. Also try tricks like wrapping tape and solder around the boring bar where it does not enter the hole. Wrap a few layers of electricians tape, then wind the solder (the stuff you get in a coil for doing copper pipe) on as tight as possible and cover with a few tight layers of tape. The idea is to try and kill any resonant vibrations in the boring bar.

I agree with the speed try slowing it down. I have a part that is 6061 Heat treated and its harder to machine than my 4140 tool steel. "Slow your RPM down your running to fast."

[SRT Mike]

Thanks for the info guys - the other job I use this boring bar for I was running at around 750RPM and the finish was pretty good, although surprisingly it sort of howled a bit during the cut (which usually means chatter which means crap finish - but it came out very nice - and it was with proper mix of coolant, so I am not sure if it was just chips getting stuck or what - but whatever).

The boring bar is held very tightly and it's as deep into the holder as it can go while giving the length I need. The insert is a positive rake polished CCMT and it's brand new, and I've tried a couple so I don't think it's the insert.

I think it's just the speed I am running it at on that size bar, I'll back off on RPM's and I will check to see how much a larger boring bar I can use on this job. I just hate changing out tools if I don't have to, since we run low volume / high mix which means a lot of changeover.

I got a note about PCD inserts. Any of you guys find them useful in this sort of application? I am not sure of the price, other than "a lot" but if they last a long time and give a great finish it may be worth it - although I am sure that a larger diameter bar + lower RPM's will solve my immediate problem. I'll try the latter first, then look into the former

Thanks!

[chrisryn]

I recently brought this problem to my iscar reps and they said for this type of aluminum when you need a good surface finish a PCD insert is the way to go. They are high dollar though.

[Mike Stevenson]

If the aluminum is very "gummy" You need to leave a lot of material for the finish pass and high RPM. The heat generated will give you the shiny finish you desire.

[DareBee]

Originally Posted by chrisryn I recently brought this problem to my iscar reps and they said for this type of aluminum when you need a good surface finish a PCD insert is the way to go. They are high dollar though.

Yup - It can be hard to justify $90 for 1 cutting tip.

[K&Y]

Originally Posted by DareBee Yup - It can be hard to justify $90 for 1 cutting tip.

First off, if you shop around, you'll see that $90.00 isn't necessarily the price of a PCD insert for this specific application.

Now, if you are in a production environment, and are using, let say for arguments sake, 30 carbide inserts/month (between $8-12 a piece), and getting sub-par results. Is it worth it to pay a little more for ONE insert that will outlast it's carbide counterpart 100-300% longer and still give you the option to re-sharpen the edge at a fraction of the cost of a new PCD insert?

If you are doing a one-off piece and want the best finish, you have to weigh the pros and cons of investing a little money to get the results that you need, or stick with the old carbide solution.

Aerospace, automobile, and plastics manufacturers have long understood the advantages of using PCD, and have actually saved more money in making the switch.

Unfortunately, most folks have the same reaction as you when looking at the initial price and don't look farther down the road, or how much they've been spending on throw away cutting tools.

[msomerville]

If you are doing low volume parts I would stay away from PCD. There is no reason that you can't achieve the finish you need with the right insert and boring bar. There is an insert I use from www.toolmex.com it is a ccgt-ak high polish insert that might do the trick with a slightly bigger boring bar. Really you should be able to get it with the size you have.