Problem drilling small holes

[Steve Seebold]

How deep were the holes? Blind or through holes?

The holes were through 6061 aluminum ,375 thick. I used 4500 RPM G83G98X?Y?Z-.45R.1Q.075F15. I probably could have used deeper pecks, or a higher feed rate, but that worked for me.

[beanbag]

So how did the holes turn out? Does the shank of the drill fit back in? Is it bellmouthed at all?

[Steve Seebold]

So how did the holes turn out? Does the shank of the drill fit back in? Is it bellmouthed at all?

Holes came out great. No bellmouth, nice straight holes.

I also did some parts last week that had a .125 hole, 4.5 inches deep. That was a trick because I drilled in to a pitce of 7075 aluminum that is .188 thick, so there is no room for the drill to walk sideways. It took 7.5 minutes to drill that part. Almost 6 minutes just to drill the deep hole. And I had to do 130 of them.

[beanbag]

I got excellent results when switching from a standard drill to a parabolic drill with a 0.125" hole when drilling through 1/2" 6061-T6 aluminium plate.

What does "excellent result" mean? And what is a "non-excellent" result from a regular drill?

[tbaker2500]

When I drill on a manual mill, I am able to pull a continuous chip. On the Tormach, I often get these small broken chips. Sometimes these chips cause clogging or rubbing, so the hole turns out bellmouthed or oversize. Specifically, I am talking about using a .100 drill, running 5k rpm (or a bit less) in aluminum and feeding at 10 ipm or a bit more or a bit less. That should give about the right chip load for drilling. Is the problem that the Z step rate isn't smooth enough relative to the time it takes for the drill to make one rotation?

When I use a larger drill like 3/8 I am able to pull a continuous chip just fine.

I use flood coolant in this case.

I pull a continuous chip in 6061 T6 with a standard jobbers bit, #9 drill 2400rpm 7IPM, if I recall the speeds right. But I still need to peck if the hole is deep, it can still clog the flutes.

[TXFred]

And what is a "non-excellent" result from a regular drill?

[beanbag]

An update on my parabolic drilling experiences. Yesterday I used a 5/16 parabolic drill (Guhring 549 series) to make a deep hole on the manual mill. I was very impressed that I could do one continuous plunge, without pecks, all the way until there was only about 1/2" worth of flute left. The drill just shoots small chips out the top of the flutes. (which in retrospect matched my experience in post #10) So in fact small broken chips is what you want with this kind of drill after all, which if I think about it makes sense. A "normal" drill tends to make long stringy chips, which is partially why they clog easier and need peck cycles.

I am still a bit apprehensive about doing a g81 on the Tormach, though. Sometimes, the flutes still clog up a little bit, and you can feel that on the manual mill with a little more drag and vibration.

Anyway, thanks to Don and Steve for mentioning this type of drill.

[esmondperry]

For the small hole drilling and you have to use the low rpm like 2k per rpm or lower...
So, your problem solved for it...

[riabma]

I have done a lot of small holes with the Tormach in aluminum with great results:

Diameter: 1/16"
RPM / Feed: 5100 / 8.3 ipm
Drill Peck: 1/3 of diameter
Tool: Low Helix Carbide
Depth: Up to 1"

Of course, center drilling before...

I hope it helps.

[Spinnetti]

looks like I need to do more research on this.. I have a part I'm doing now with 1/8, 3/16, 3/8 and 1/2 holes, 3/8 deep, flood coolant, no center drill, with one cut each (no peck), using plain ole' black drill bits in collets on my series III. Except for the 1/8, I think I'm running all the bits at 5100 speed and at least 16ipm... (will have to confim).... so far, it zips right through... The 1/8 and 3/16 size are silent when it cuts, though the 1/2" scares me a little and throws chips. The 1/8" I think I'm running about 4100rpm? I have lots to learn though, so this is an interesting discussion... I'm using gwizard to set my starting speeds and feeds, then tweak based on conditions from there. So far, clean holes, on size with no broken bits, though only have run a handful of parts. (seems to match Steve's findings pretty close?)

[Steve Seebold]

I do holes all the time that are .090 to .159 diameter, 4.5 inch minimum depth. I use ONLY Guhring drills. I don't even mess with anything else.

Yeah, Guhring drills are close to double the price of any other drills, but if I can drill 150 1/8 inch holes in the end of a piece of 3/16 aluminum, and not have any break out the side, it's well worth the difference.

I know of other guys who try to do what I do, and they will lose 1 part out of 6 because the hole breaks out the side of the part. The next job I do, I need to drill a .090 hole 4.5 inches deep in the end of a piece of material that is .156 thick.

[tbaker2500]

Thanks for the heads up, Steve. I'm going to need some precise holes soon, I'll try out Guhring. Where do you buy them from?