Drilling and tapping 200+ 3/8" holes in 3/4" aluminum

By chance I just finished drill and tap to 3/8 on four holes in AL

Karl

sorry you had two more queries.

I used a solid holder, your floating holder would be nice.

Spot drill if you need to hold +/- .002 location, stub drill maybe +/- .005, regular drill maybe +/- .010 or worse. So how accurate determines answer.

Karl

That depends on the drill and the material. HSS drill? Maybe 2500 RPM and maybe .005 per rev feed. That is a bit conservative, but I'd prefer to finish without a lot of tool changing. Pecking once will probably be sufficient.

Be wary, though, of scoring "good deals" in material. If this isn't cast tooling plate, but some soft sticky stuff more akin to 1100, you'll have your hands full. Use a cutting fluid.

Absolutely, if nothing else, done properly, they provide the chamfer for the finished thread.

Sure. Go for it. However, again, if you have inherited some suspicious material, say one of the 6xxx materials.... you'll dull taps VERY quickly and a tap burner or scrap will be in your immediate future.

Not bad. 80 rev per secons and 0.005 per rev means 0.4 inch per second.

Would the stringy chips want to wrap around the drill bit?

I will use flood coolant in large amounts.

his plate alteady has a few smaller holes drilled and tapped.

Great. I am thinking, use a spotting drill, and drill a full diameter hole that is perhaps 1/8" deep. That would provide good centering.

Well, it is already tapped, so it is tappable.

ix

I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill.

Pretty cool. You feed 5.1 is how many inches per second?

Someone suggested 0.4 IPS, which makes some sense to me.

That's 5.1 IPM. I just looked at the math, probably could have doubled the feed. Only four holes, chips were feeding, don't f*ck with it.

Karl

Just trying to do the math. 5 IPM, means one 1" hole drilled in 12 seconds, so it amounts to about 20 seconds per hole with rapids and everything. 200 holes, means 4,000 seconds, a little over an hour. Probably can run unsupervised. Not too bad.

How bad were the chips?

If you use 60 degree center drill and go to a depth of half the hole diameter of the 3/8 thread diameter the finished hole will have a nice chamfer on it with no need for any deburring.

John

How frequently do you break taps? If you're not an utterly reliable tapper, you'll never be able to complete this job. Consider that if your workpiece is ruined by breaking a tap, then you must succeed at all 200 in a row. For a 90 percent chance of success, then, each individual hole must be tapped with a 99.95 percent chance of success.

If you break a tap, say, once every hundred holes, then you have an 87 percent chance of failure on this piece (1.0 - 0.99**200 = 0.87).

Now you know why these cost $$$$:

Is a "spot drill" the same thing as a "center drill"? (it kind of sounds like it, from Karl's info here.)

Thanks, Rich

This makes me wonder: Is there a machine where a machinist could make one part "by hand", i.e., in the normal way you'd use a regular mill or whatever, but where the machine could record the machinist's actions, and then "play them back" for the next part? Or is it only possible to drive an NC by writing a string of textual commands?

Thanks, Rich

On Sep 26, 10:23=A0pm, Ignoramus24898

If I were doing this on a manual mill, I would spot drill with a drill whose diameter is about the size of the web of the drill used for the hole.

Dan

No, they are different. A spot drill looks like a drill bit with a special grind point.

I had no trouble with my mystery metal AL. Some AL is a stone bitch to feed the chips up the drill bit, others work great. As nearly all my metal falls in the mystery metal class, i can't tell you which grade is best.

You should feed maybe twice as fast as my small run.

Karl

My control has a "teach" mode to record points but you still eidt to make a program. I never used one but the bridegeport protrack was supposed to do this.

Karl

Karl, thanks. I will try on some aluminum junk that I have, first.

Tapping, as Richard noted, may be a challenge.

What tap would you recommend for this (tapping aluminum)?

Thanks

Richard, I was hoping that I would tap on my CNC mill, so whatever process I do, would be repeatable and not as random as manual tapping.

For aluminum, you may want to use a Thread Forming Tap, instead of a Thread Cutting Tap...Since you will be using coolant/cutting fluid, the going will be much easier, and the thread will be stronger. A thread forming tap has the additional advantage of no chips.

_kevin