Deep holes in 6061

[racerdog]

Trying to drill .250 hole 2.6 inches deep in .500 outside diameter 6061 aluminum.
As you can probably guess the drill walks and I end up with a hole about .020 off center.
I've tried drilling on a manual lathe and on our CNC mill.
I get a little bit better results on the CNC by using a .025 peck cycle and plenty of coolant but the hole is still unacceptable.
The boss has got hundreds of these things to do.
I center drill each part and drill with a 135 degree jobber drill. No special grind on the drill.
Is there a better drill to use other than the one I'm using now?
If so where would I get one?

racerdog

[Geof]

Try using a 3/16" cutter to interpolate a .250" hole maybe 1/2" deep then go in with the drill. Also maybe try two drills; go as far as possible with a stubby then finish off with a longer one.

[motomitch1]

single flute gun drill

[chuy]

there it is right there....135 is no good for deep hole drilling
use a 118 deg. get an osg gold drill and you can eliminate the spot drill make sure your peck is at least deeper than than the drill point...if you have a cnc run it 2900 rpm with 16 ipm feed and a peck of .075 and you'll be fine...

[mmachining]

Use two ops. Drill past center then flip and do the other side.

[racerdog]

Thanks guys. I'll try the OSG drill. I remember we got some stashed somewhere.

racerdog

[ctate2000]

Check your machine alignment and set up also. A hole that starts in the wrong place will stay in the wrong place. You may not be walking.

[Paul_S]

135 deg split point drill will in fact work better than a standard 118 deg drill.

Also a parabolic drill 135 deg or 130 deg work very good. And can drill faster than a standard drill.

But if the head of the machine, drill press or mill, is not square to the table you will have a problem.

A check would be to place an indicator in the spindle and to tram the table. If the table is square to the spindle, the indicator will keep the same dial reading. If it dial changes as you tram in a circle, that is how much your drill will seem to walk. Because you would not really be drilling square to the table.

You will need to set up some kind of work holding to keep the part square to the spindle. (Assuming that the spindle to the table squarness can not be readily adjusted or fixed.)

I once had to drill .128 hole 6" through a part. The head of the VMC Mill was not square enough to make this work, using square to the table work holding. The holes wouldn't match, be aligned in the middle. Thankfully, Engineering changed the design so the part just needed to be drilled a shorter distance on the ends. Drilling 6" wasn't the hard part. Drilling square was.

[chuy]

nope... your wrong parabolic aren't standard drills and they much more costly than a 118 deg. if your a tool programmer I wouldn't expect you to know that.

[kalmah]

1) I would use 118° center drill

2 ) I think that the drill for your work should have:
- Smooth coating with low friction coefficient (DLC coating as exemple)
- 30-35° helix angle
- Special flute design for a good chip evacuation

http://www.nachi-fujikoshi.co.jp/web/pdf/2292.pdf

PS: I 'm not purchaser of Nachi !!

[KEYTEEM]

Racerdog,, how did you make out with this problem,
what did you do to solve it?

[Paul_S]

Originally Posted by chuy nope... your wrong parabolic aren't standard drills and they much more costly than a 118 deg. if your a tool programmer I wouldn't expect you to know that.

I never said a parabolic was a standard drill >

Also a parabolic drill 135 deg or 130 deg work very good. And can drill faster than a standard drill.