Any ideas?

I have a piece of 2.5" 6061. I drill a 1" hole 2.3" deep. Then I bore the entire thing to 1.25", then I bore the top 0.75" to a width of 1.9".

The main problem I am having is that when I am boring out the hole, I am getting long stringy bits of aluminum that fly around, curl up around the boring bar, get all wrapped up and lead to a crap-tastic surface finsh as they all get in the way of the boring bar.

Specs are...

2500RPM
0.100 depth of cut
0.005IPR
1/2" boring bar (I know I could use larger but I need this for some other jobs)
21.51CCMT insert that's positive rake and polished (made for aluminum)

I do not have coolant through the boring bar.

It seems the problem is that it's just not effectively breaking the chips. If the chips were breaking I could mess with the coolant nozzle to make sure it's blasting into the bored cavity and flushing the chips out, but when it turns into a bit string and wraps around the bar, it turns into a big ball that looks like steel wool and impedes the coolant flow as well.

I am thinking maybe its insert wear (doubt it - almost brand new insert)
Possibly my feed/speeds are off?
Maybe I am taking too big a cut? Too small a cut?

Any opinions are welcome!

what does the mfg. say to run that particular insert at?
seems really slow with way to light of a feed rate.
mash the meat to that thing, and i bet your problem goes away.

Use the G74 Face Groove Pecking canned cycle. You can adjust both the length of peck and the amount of retraction; you do not need to withdraw completely from the hole just pull back a few thou. You can also adjust the X increment so you have two lines of code that bore all the way from your drill size to the 1.25" size then another two lines to go to the 1.9".

I got the inserts from MSC - it says "Broussard Enterprises, LLC" on the case but I can't find them by doing a web search.

I also am facing and turning an OD with a CNMG 432 insert at around the same speed and its taking forever. Its my first time running this program and aluminum so I could be way waaay off on speeds. A machinist next door told me that he never exceeds 1/2 the nose radius for the step-over so I was just sort of guessing here.

I was hoping I could crank that sucker up because the cycle time is long.

Can someone suggest a good range for roughing and finishing? I get an almost mirror shine on the OD with 0.003IPR 0.005DOC 2500rpm, but it's a pretty slow pass. I just cranked it up to 0.005IPR 0.100DOC for roughing and left it like that... but if I can go faster I will.

Use the G74 Face Groove Pecking canned cycle. You can adjust both the length of peck and the amount of retraction; you do not need to withdraw completely from the hole just pull back a few thou. You can also adjust the X increment so you have two lines of code that bore all the way from your drill size to the 1.25" size then another two lines to go to the 1.9".

Geof do you happen to know if the Okuma OSP5000 control supports all 'standard' Fanuc G-codes?

The manuals for this machine look like they were written in Japanese, then translated to Latin by a dyslexic orangutan, then re-translated into Engrish by that orangutan's moron brother. It's not that they are imprecise, they go into painful detail on some stupid things (like how to calculate whether a tool in the turret will interfere) and gloss over things that are kind of important (like how to actually program a G2/G3 command correctly).

They manual just skips over a bunch of g-codes like most of the canned cycles. If the Okuma is standard Fanuc I know I can find the commands/parameters online :)

I think that you could use 0.015 IPR instead of 0.005, or even more.
is your boring bar too weak? is hanging out too much?

I think that you could use 0.015 IPR instead of 0.005, or even more.
is your boring bar too weak? is hanging out too much?

Its about 1/2" shank on the boring bar (tapers a little at the neck) - it's an 8-2 size. It's hanging out around 2.5" from the holder, although I am boring down 2" so I think it ought to be rigid enough.

I will try 0.015IPR and see how I do. Those little CCGT 21.51 inserts just look so.... dinky... next to the CNMG432 size that I guess maybe I was nervous to really push it in case I break something. I also didnt have much of a reference point to start with - but this is a good one, thank you!

For roughing aluminum on the OD you can use over 0.020 IPR, 0.200 DOC, and speeds above 1000 sfm (I would use G96 instead G97).

2.5 od on aluminum, i'm gonna say go waaaaaay more rpms, probably max.
as far as feed on the od turn, assuming no crazy finish callout, .01 per rev
even with a big depth of cut should give a pretty good finish.
just remember aluminum is a soft material, in order to break a chip, it
has to be pretty thick, .01 per rev is pretty conservative considering
i'm not sure of your machine, rigidity, etc.
hope this helps

2.5 od on aluminum, i'm gonna say go waaaaaay more rpms, probably max.
as far as feed on the od turn, assuming no crazy finish callout, .01 per rev
even with a big depth of cut should give a pretty good finish.
just remember aluminum is a soft material, in order to break a chip, it
has to be pretty thick, .01 per rev is pretty conservative considering
i'm not sure of your machine, rigidity, etc.
hope this helps

Well max RPM's is 3000 but it's got a gigantic chuck on there that I dont like to spin more than 2500 :)

The machine is plenty rigid, it's an Okuma LC-40 with a 60hp spindle motor. All the turning holders are 1.25" and I am holding the part in machined soft jaws.

I will try cranking up the speed to max and going with 0.01IPR and work up from there instead of 0.005.

At least I know .005 gives a beautiful finish for the finishing passes at 5thou DOC. I'll keep pushing and see how I do :)

60 Hp?

That's a lot of machine for little .100 DOC on aluminum!

Geof do you happen to know if the Okuma OSP5000 control supports all 'standard' Fanuc G-codes?.....

The manuals for this machine look like they were written in Japanese, then translated to Latin by a dyslexic orangutan, then re-translated into Engrish by that orangutan's moron brother....

Can't help you on the capability of an Okuma. And I am tempted to report you to the Orangutan Antidefamation League :D.

Do you have a description for G74? I can screen capture a page from the Haas manual that describes it if you like.

60 Hp?

That's a lot of machine for little .100 DOC on aluminum!

better too big than too little :)

Can't help you on the capability of an Okuma. And I am tempted to report you to the Orangutan Antidefamation League :D.

Do you have a description for G74? I can screen capture a page from the Haas manual that describes it if you like.

Thank Geof, I was able to find a description online.

Ironically the Okuma manual has at least 20 pages devoted to tool radius compensation, and a single half-page on the entire G74. It lists the parameters and says things like "I - the amount to step with each move". Gee very helpful :)

But with the online help I should be able to nail it down. Thanks!

hmmmmm.
so me's an orangutan?
we be havin a league?
who we be playin?
da raiders?

da riverrat

I bumped up the feed to .010 IPR, 2500RPM on the boring - MUCH less stringing of chips but still some. Pushed it up to 0.012IPR and I got no stringing, but it was sort of singing (a high pitched screeching noise). I'll mess with it a bit more, see if I can get it any better but if what I got now is what I have to live with, it will be OK.

Cycle time was also waaaaaay faster (thanks on that front!) and I turned the original OD with a .015 stepover on the OD roughing with the CNMG 432 AL bit, finish is actually pretty damn good. It's getting turned on a 2nd op anyway so no biggie..

Thanks for the help

If you're interested, you can calculate your finish for your finish pass. .0567 x sqr(tool radius) x sqr(AA finish wanted / 125) = ipr for finish. If you want an RMS finish use .0542 instead of .0567.

I bumped up the feed to .010 IPR, 2500RPM on the boring - MUCH less stringing of chips but still some. Pushed it up to 0.012IPR and I got no stringing, but it was sort of singing (a high pitched screeching noise). I'll mess with it a bit more, see if I can get it any better but if what I got now is what I have to live with, it will be OK.

Cycle time was also waaaaaay faster (thanks on that front!) and I turned the original OD with a .015 stepover on the OD roughing with the CNMG 432 AL bit, finish is actually pretty damn good. It's getting turned on a 2nd op anyway so no biggie..

Thanks for the help


That screeching noise is called chatter. Not good for carbide inserts. So what if you need the 1/2 inch bar for another job. It isn't that hard to reset the geometry for it. Good thing you are running aluminum. That small insert couldn't take anywhere near that DOC or speed and feed in a harder material without breaking and wiping out the tool. Do yourself a favor, and stick a 3/4 inch boring bar in the machine.

How much material is coming off the OD? .015 stepover is ridiculously light for roughing. Any catalog I ever read said to bury the insert at least 1/2 the tool nose radius of the insert for finishing. I don't follow that rule. Normally I leave .005 or .01 DOC for finishing, even on aluminum, but it does cause stringing. However, since this part gets finish turned in another operation, there is no need for such a light DOC or slow feedrate for the finishing pass. Normally I am holding tight tolerances and a good finish, and these practices are a carry over from running other materials. Aluminum jobs are few around the shop I work in.

I think someone mentioned using a G96 instead of a G97. Don't bother at those diameters. Run the machine as fast as you feel it can safely run with that size chuck.

BTW, I agree with you about the Okuma manuals. Not very "friendly". Hardinge manuals are MUCH better.