Need Help!- deep, small hole drilling in aluminum

[Fala_Man]

I need to drill 112 thru holes .0197 diameter in 6061 .325 deep.
I have CRT carbide drills. I have 20,000rpm capability on
the machine. Any suggestions for drills, speeds and feeds,
coolant or oil, technique's???

Thank You

[John Welden]

Originally Posted by Fala_Man I need to drill 112 thru holes .0197 diameter in 6061 .325 deep. I have CRT carbide drills. I have 20,000rpm capability on the machine. Any suggestions for drills, speeds and feeds, coolant or oil, technique's??? Thank You

Few thoughts

Not sure I'd bother with carbide, but I haven't had to drill that many holes with hss. HSS might be easier. I drill hardened stainless (17-4 h900) with coated hss.

Going 20x the diameter isn't optimal. Are all the holes in one part? If not than good, because you're likely to break a bit going so deep.

The problem with running high RPM is that the bit can whip out from the centrifugal force. Of course it depends on how long it is.

Sometimes I slow the rapid down and set the plunge clearance a bit high to give the bit a chance to cool and shed any chips.

You can't blast the coolant or the bit will deflect away. For aluminum, normal coolant should work just fine.

It's hard for me to say how fast to run because I don't drill aluminum and it's one of those things you have to play around with. Every job and machine is different. Maybe your spindle vibrates, maybe your bit is running out, maybe you didn't spot drill very well, maybe your coolant is bad .

You'd be surprised how slow in RPM you can run those tiny bits. You don't have to go mach 5.

In the stainless I might peck around .004 or so. I'd rather stay on the conservative side and get the job done.

I'm always surprised how well the tiny bits do. It's hard to believe they can drill anything.

[iamstink2k]

MIGHT HAVE BETTER LUCK DRILLING ABOUT .1 DEEP WITH A STUBBY CARBIDE DRILL THEN FINISHING THE HOLE WITH A LONGER DRILL. (HS OR CARBIDE)

PROLLY SHOULD RUN BOTH HS AND CARBIDE AT 20,000 RPMs
AS FOR FEEDS 100IPM IS AT A .0005 CHIP LOAD, SEEMS A LITTLE TO FAST THOUGH

[bostosh]

more info needed, all in one part? have you ever done small holes?, etc. I could do this on a jig borer manually. (done it before) under 5 minutes per hole. no broken drills.

[gankoji]

Well, The best way to do what you want to do is what someone suggested before. Start the holes with a center drill, if you can get one that small. Then, Drill a pilot hole with a normal SML drill for that diameter (should give you between .080/.100 cutting depth). Then come in with your long drill and finish the job. 20,000 RPM will do well to cut down cycle time, however you need to take incredible care to make sure the TIR of your toolholder is within .0001 or less. Any more and you will have unacceptable deflection/side load in that small of a drill. Also, a balanced toolholder will probably be necessary if you plan on taking a 20:1 drill that small to 20k RPM. I personally wouldn't feed the drill at anything more than .001/.002 chip load, which would give you 40/80 IPM @ 20k on a 2-flute drill. The shorter drills you could push a bit more, but it would be wise to start low and work your way up, instead of the other way around. Hope that helps you out.

[jrobson]

The carbide should help, if you can get a single flute bit that size even better in Aluminium, 20000rpm is too high, run much slower to start with (1000rpm) then pick up from there, don't feed too slow either, use a small setup piece that you can break the bits into and you will quickly find where the best performance is, set your peck at no more than 3 x diameter maybe start at 2x, we've done holes like these in brass, make sure you have spare drills untill you find the sweet spot, hopefully you didn't quote that low it's going to take a little bit of time. Good luck.