Need Help!- drilling 6061 aluminum

[cuz1007]

I need to drill a hole from bar stock 1.049'' diameter and a lenth of 4.0'' I tried a spade drill, no good, looks like a cork screw, I also tried a fixed drill at 1 inch diameter, then offset the drill .030 in x then ran a boring bar in no good, too much chatter. does anyone have any suggestions, as to speeds and feeds or spade or fxd drill???? This is on a machining center lathe. please help, running scrap?????

[sti2011]

The option you took, drill 1.0 dia, then finish bore to size should work fine. More info is needed though as to what type, dia, inserted or no, boring bar is being used. 4 inches deep is really not bad by any means but I would probably stick to a bar that is .625 dia min to keep your overhang ratio reasonable.(depth of hole divided by bar dia)
I would also take a rough pass then a finish with the bore bar.
Offsetting a drill diametrally (standard twist I asume) is probably never a good idea unless you are working with some really forgiving mat. like plastics.
If you have an insert type drill then that is the way to go as lots of them can be offset diametrally as well as be used for some boring as well.

[cuz1007]

thanks for your input, can you suggest any speeds and feeds for drilling aluminum?? the drill is a fixed insert drill, and the bar is .750 in diameter that has a zero degree lead. i'm afraid if i use a .625 diameter bar i will chatter even more?? Our cnc wizzard as we call him just retired, i'm sort of on my own in the shop!!

[g-codeguy]

Originally Posted by cuz1007 I need to drill a hole from bar stock 1.049'' diameter and a lenth of 4.0'' I tried a spade drill, no good, looks like a cork screw, I also tried a fixed drill at 1 inch diameter, then offset the drill .030 in x then ran a boring bar in no good, too much chatter. does anyone have any suggestions, as to speeds and feeds or spade or fxd drill???? This is on a machining center lathe. please help, running scrap?????

I'm a bit surprised the spade drill isn't working. Could you give your speed and feed values? Also are you getting a nice coolant flow thru the drill body? How deep can you drill with the spade drill?

I had a similar job where I was drilling a .969 hole a little over 3 inches deep. (This was on a lathe.) The insert drill was pushing sideways!!! Forget what I was running it at. I used one of Kennametal's drills with the solid chunk of carbide on the front. Similar to a spade drill. Forget the name of the drill. Can look it up at work tomorrow.

Anyway I believe I ran it at S2000 and F.016. Could have gone higher on the feedrate, but in was only taking a few seconds to drill, so I figured why push it harder.

[sti2011]

Probably too late to be of any help but, provided that your bore bar is positioned properly ie: on center above or below as the tool dictates. You can get away with most anything. I personally always run bore bars a little above center as as they load the depth of cut gets lighter and they chatter less if not at all. Below center will deflect even deeper into the stock and cause more chatter. Aluminum is really forgiving as to feeds and speeds and I suspect that with a .75 dia bar the problem you are having is more a set-up issue. As to an exact feed and speed there is none with alum or any other material for that matter. These are all based on each situation especially when boring. The more the overhang the slower the speed typically. I will turn at 1500-2000 sfm which usually means I max out on spindle speed before I get there typically, as lots of our work is below 4.0" dia. As far as boring on relatively short overhangs I start at 1000sfm and work it from there. Bearing in mind though I have inserts and tooling specifically for alum. (up-sharp, polished and ground)As well as for other materials. Without knowing the specific brand of tool, insert or the actual set-up. Try the really safe 1200rpm and a feed of .005 or more until the chip breaks on roughing (.06doc) and step it up to 1500rpm and a feed of .003 for .0078r and .005 for .0156r for your .003" per side finish cut.