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

I bought a couple of 3/4" thick aluminum fixture plates.
formatting link

It was a local sale.
I would like to drill and tap them with 5/16" drill and 3/8" tap, say
spaced at 1" interval. That makes for about 200 holes to be drilled
and tapped on my CNC mill.
Some questions.
1. What is the best way to drill aluminum with 5/16" drill bit, making
through holes. What RPM and feedrate and how often to peck.
2. Do I need to center drill those holes first? It is not really a big
deal, just some more G codes.
3. For tapping, can I safely use a ER colleted floating tap holder that has a
little bit of vertical internal travel. Like this one:
formatting link

Reply to
Ignoramus24898
Loading thread data ...
By chance I just finished drill and tap to 3/8 on four holes in AL 1.25" deep. I used G81 (no peck) feed 5.1 speed 2100. Got thick chips that fed out well and broke every two inch or so. Used my coolant mister at a heavy flow.
Karl
Reply to
Karl Townsend
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
Reply to
Karl Townsend
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.
Reply to
Gene
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
Reply to
Ignoramus24898
I will use a spot drill indeed. Full diameter holes with spot drill, perhaps 1/8" deep, to provide guidance for the regular drill.
i
Reply to
Ignoramus24898
Pretty cool. You feed 5.1 is how many inches per second?
Someone suggested 0.4 IPS, which makes some sense to me.
i
Reply to
Ignoramus24898
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 fuck with it.
Karl
Reply to
Karl Townsend
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?
i
Reply to
Ignoramus24898
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
Reply to
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 $$$$:
formatting link
Reply to
Richard J Kinch
Is a "spot drill" the same thing as a "center drill"? (it kind of sounds like it, from Karl's info here.)
Thanks, Rich
Reply to
Rich Grise
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
Reply to
Rich Grise
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
Reply to
dcaster
No, they are different. A spot drill looks like a drill bit with a special grind point.
Reply to
Karl Townsend
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
Reply to
Karl Townsend
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
Reply to
Karl Townsend
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
i
Reply to
Ignoramus21149
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.
i
Reply to
Ignoramus21149
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
Reply to
karchiba

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.