Results 1 to 12 of 12
Thread: Drilling Copper
03-11-2008, 02:37 AM #1
SImple question. Really.
How the @#!%$&@ do you drill Copper?
This is Amcoloy 97, gotta put 2 holes each of .140 dia @ 1" depth and 6 each of .203 dia @ 1.35 depth.
I'm on part #2 and so far used up 2 #28, 3 #7 drills and exactly 3.2 years of my life expectancy.
Considering there is 58 more to go, I'll be dead by 9:25 AM tomorrow.
03-11-2008, 03:06 AM #2
I'm guessing you are working the night shift, and since it doesn't look like many other people are awake. I have some copper experience, but quite a bit in aluminum bronze. Its nasty abrasive, and it grabs.
So, slow, and wet, and since it grabs, a neutral rake on the end of your drill, as in, get rid of the sharp positive edge, stone it flat, not the relief on the bottom, but the actual cutting edge.
I may be totally wrong, but I'm sure at some point somebody will wake up and give you some more info.
03-11-2008, 05:14 AM #3
Think a half-round drill would work in copper?
I have an occasional copper job that requires a 1/8 drill about 1.5" deep, and the strings get stuck to the drill and need to get pulled off after every hole.
I had the same problem with a plastic job I was running, and switched to a half-round drill and the chips simply fall into the chip bed, worked great.
03-11-2008, 10:46 AM #4
What Bobw said; neutral cutting edge. I've even done some with negative edge, about 2 degrees.
03-11-2008, 11:00 AM #5
I probably don't know enough to give valid advice, but I did a bunch of .120 dia holes in copper near 1" deep recently. I ended up using a garr carbide jobber length drill, and then cranking up the RPMs. I was running about 7K with 7ipm of feed. Turned out that the RPMs were my friend as that caused the chips to evacuate instead of balling up on the drill and starving the hole for coolant. I flinched as I started cranking up the feed, but the feed helped to break up the chips. I am not sure what grade the copper I was using was and how it would compare to yours, but maybe this will help you a bit. I called Garr and got good help with their tech support. Carbide was the answer for me and more feed. I did use a peck drill cycle even though the tech said to not go to a full retract as it chips the leading edge of the drill on re-entry, but I didn't have the guts to change that. Good luck.
03-11-2008, 11:23 AM #6
Oh, hell. Night shift, day shift, trash run, accounting, complaints department....
Just got back with a set of different drills, ranging from standard black to high spiral coated. I've just discarded every single bright drills from my arsenal, as to date have not found anything that can be drilled with them.
Slower speed, less upsharp tip..... I'm going to town in a couple of minutes.
03-11-2008, 01:52 PM #7
I agree with grinding off the positive rake lip on your drill. Here's a suggestion: Set up the drill in a simple (small) drill press and try drilling a part there. The drill press will give you some measure of what feed will or won't work as it will provide you with some feedback as to cutting force. On a VMC with such a small drill; one minute it's there and the next minute it's broken.
03-11-2008, 01:55 PM #8
I ran a job cutting c110 copper a little while back, granted the holes were about .265 in diameter, I had good success with OSG EX-SUS-GOLD List 1100. I would call and talk to their tech, but if I remember right my RPMs were around 1100 with a feed rate around 12ipm. It is important that you feed fast enough to get those chips popping. I was able to get around 500 holes per drill.
03-11-2008, 03:03 PM #9
Not sure if this was the right way to go, but hey, try 'till something works.
Got a Titex parabolic drill and went to 2000 RPM .002 IPR feed.
Obviously the chips don't break or fling off the tool, but with the small feed they are soo thin that the drill can carry them out and bunch them up at the neck where they cause little trouble.
So far got through 20+ parts and the holes appear to be fine, on size and with a very acceptable finish.
Did try to go higher feeds and some of the chips did get smacked around from the rotational forces, but they actually broke off at the welding point so the tip was still loaded.
Considered the duller tip also, but wondering how straight would the hole be. Remember this is only .140 and .203 dia and I need less than .005 location variation on the other side.
03-11-2008, 03:33 PM #10
My experience drilling deep holes in c110 resulted in using TiN coated parabolic drills. Richly mixed coolant, pecking, and listening for the first indication of squeaking. Not using coated drills was a waste of time and money.
03-11-2008, 09:54 PM #11
TiCN coated cobalt or carbide. copper is very dense. we used to put parts in a deep freezer run heavy then finish mill later. heavy concentrate or straight coolant, i use crisco on small drilled holes, it works best. you kinda have to push it a little any rubbing and all your doing is polishing the drill. think of it as cutting an apple yo want to slice the copper away, we always use sharper drills but we run lots of high % copper close to 78 or 80 pure. alum bronze is crappy, that stuff is like old dry bubble gum with hard nastys all inside, like a candy bar from hell.
03-11-2008, 09:59 PM #12
Hmm... Just finished them miserable things.
Alltogether 360 + 120 holes...
Did put a damper on the cycle time but if I look at all the drills I did not have to change... I guees it's worth it.