What's new
What's new

Drilling 110 Copper small holes

3t3d

Diamond
Joined
Nov 1, 2004
Location
WI
I am working on a job that could need about 105,000 1.5mm holes .390" deep in 110 copper bus bars.

The first 100 holes were a pure nightmare. Tried rich coolant, various speeds,feeds, pecks, and retract heights.

Equal numbers of M3 x .5 tapped holes.They tap nice, but again, drilling is "challenge"

Any great ideas?

Coolant fed drills a possibility? I see 1/16" coolant fed, seems like it could be crazy fragile.
Hate breaking $200.00 drills AND scrapping an expensive part.

My Google foo is week. Most searches pointed back to my previous posts on a similar job. That was #37 holes 1/4" deep.
That job went OK, but this job with 1.5mm holes is a Nightmare.
The #37 holes could have a broken drill punched out from the backside. Not these parts.
So any break scraps out the whole part.

Thanks Again!
 
Hi 3t3d:
Is everyone convinced it MUST be C110 copper?
If so, the customer is royally fucked (or should be) and (in a fair world) will have to eat whatever scrap you generate.

The customer should pay for every bar that goes in the machine, and every drill you scrap and every setup you need to duplicate.
That's what he buys for specifying such a Godforsaken shit-miserable material.
You can try cutting it with milk or some other exotic magic goo, you can have an operator babysit the machine and watch as it breaks drills, you can doodle around with speeds and feeds and drill materials and coolant through all you want; soft coppers are a nightmare to drill because the chip expands in the hole and will sooner or later twist off a drill.

I have had sphincter clenching "sort of" success with Rapidtap and very short peck increments like 0.0005" or 0.00075", but I was drilling a few holes, not a hundred thousand holes.


If C110 is not absolutely mandated, you can switch to tellurium copper.
Your drilling problem will go away.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
My default is to always call Guhring. Sorry you have a job from hell.
 
I recall drilling holes in 110 many years ago, and I would expect that we used Titex Super22's.
I don't recall having much trouble, but our holes were maybe 3/16 - 7/32 (?) and 2" deep?


-------------------------

Think Snow Eh!
Ox
 
The larger holes are not much trouble at all.
The M4 holes with the .145" drills or above, are no trouble..
But the smaller drills only last about .. so ... long, and they snap off and embed themselves into the goo.
The spindle keeps madly packing more drill fragments around the crater and the whole part is scrapped.
 
Mitsubishi MVS / MWS coolant thru drills have done everything I've asked of them and more. I think coolant thru will help you immensely.
 
So 1.5 x 10 mm holes by the K. Ouch! Several things come to mind but then I'm still not thru my first cup of coffee.
a. since chip evacuation seems to be the real problem not cooling(?) try high pressure thru the tool air, low viscosity might help flow.
b. drill larger holes and swage in an insert (maybe for both the smooth holes and threaded.
c. edm hole popper
d. punch or swage the holes which poses the problem of where the extra material is going to go. Bulge in back of bar or around the hole.
Now I'll return to my coffee; that I do know something about. :-)
 
So maybe a stupid suggestion. Many years ago I needed to make solid copper blocks 2" thick with a through hole and a 1/2-13 tapped hole. Drilled in a Bridgeport with a standard 118 degree jobber drill the holes were ragged as all hell. Got out an old Atlas copy of "How to Run a Lathe" and found the recommendation to use a stone to remove the hook from flutes by stroking it parallel to the axis of the drill. Beautiful smooth holes with no problems. This has always worked well in HDPE, PVC and fiberglass too.
 
I don’t remember the grade of copper, but we had a hell of a time with it. I wound up doing all sorts of silly things to make it work.

Like. . . Interpolate your 1.5mm hole with a 1mm endmill with tiny cpt?

First thing I would do after verifying material selection is call my guhring rep as previous folks recommended. I lean HEAVILY on my tooling suppliers. If they can’t give me technical support, I see no reason for them to exist as a “middleman”.

I called my guhring rep about a small production job with some unique, for me, challenges. He thought it was neat and drug his boss down to check it out. He went through each drilling operation and gave me specific parameters to try. They were awesome.

The “premium” price of those drills was more than worth it just for the technical input.
 
Thanks everyone.
This job is on hold for now.
Was going to have a TSC drill to test next week, but, well, not for now.

Interesting to note that the top Google results keep coming back to this forum and a previous thread on this subject.

Thanks again.
 
My "foo" comes up with endless out-of-box solutions.
Some fail.
Some work impressively.

On tiny holes of d/l problems, it might be possible to heat the copper as work advances.
Depends on the workpiece.
Warm/hot coolant c/should do it, in copper, very conductive.
This could maybe reduce rubbing and incremental heating of the drill.

On such very high nr of holes, cost and time // expected productivity is probably the critical path.
A custom tool running like 20 turbine drills at once might also be a solution.
Everything depends.
 
I've had some good results, clearing back the Drill flutes. So only about .05" of flute behind the Drill point. I've also had better luck with a very low Drill angle. 140° Drill point.

R
 
Similar to what garyhlucas posted above, I have always "dubbed" the sharp edge off the drill when working with soft copper. Just grind a small flat on the cutting edge so it is parallel to the drill axis. Essentially making the cutting edge a neutral rake. Width of the flat is about .5 of the feed per rev.
 








 
Back
Top