Advice for drilling solid copper

Emilyfinchum · Oct 18, 2021

Hello everyone. Needing some help with drilling a .062 hole into .130 diameter material on a lathe. My current program reads as follows
G97 s1000 m13;
M98p1;
T4x0.;
Z.2 s3000;
G1 g99 z-.65 f.0005;
M98p1;
I'm running on an older hardinge lathe, with barely any stock protruding from the face of the spindle and it pulls out to part length after it drills to prevent the stock from bending. Chuck pressure is all the way down to 30psi to prevent crushing. Carbide through coolant drill.
I've managed to make 1 part and the drill broke on the second. I've tried many different speed and feed combinations with no consistent luck. Does anyone have any ideas what to do to get this thing to run consistent? Thanks in advance

crossthread · Oct 18, 2021

It kind of depends on if you have the equipment to change the profile of your carbide bits. Copper is gummy and grabs pretty easily. That is probably the reason you broke your bit. It is a common practice to dub the bit when drilling copper to keep it from grabbing. If you don't have the equipment to change the profile of your carbide bits then I would go to a standard bit and dub it.

jim rozen · Oct 18, 2021

What is the top spindle speed on this machine?

Emilyfinchum · Oct 18, 2021

I am honestly not sure

Emilyfinchum · Oct 18, 2021

Thanks! I'll give it a shot

mhajicek · Oct 18, 2021

Might be better off with a cobalt drill instead of carbide.

Mtndew · Oct 18, 2021

Emilyfinchum said:
G97 s1000 m13;

That's 16 SFPM. WAY too slow.
You need to spin at least 4,000rpm if your machine can go that fast.

jim rozen · Oct 18, 2021

Mtndew said:
That's 16 SFPM. WAY too slow.
You need to spin at least 4,000rpm if your machine can go that fast.

I think 100 SFPM is about right. For a 1/16 dia drill that's about 6000 rpm

0.062 X 3.14 = .198 inch circumference = 0.0165 feet circumference

100 ft/min / 0.0165 feet = 3030 rev/min

What's the max speed on the lathe?

Woodeye1 · Oct 18, 2021

I had a somewhat similar situation. Went to straight flute drills. That took care of it for me

Illinoyance · Oct 18, 2021

Woodeye1 said:
I had a somewhat similar situation. Went to straight flute drills. That took care of it for me

Are you referring to a half round drill?

52 Ford · Oct 18, 2021

Illinoyance said:
Are you referring to a half round drill?

McMaster-Carr

Maybe these.

52 Ford · Oct 18, 2021

Thought it was standard practice to "brass off" the edges on a twist drill if you're going to drill something soft like copper. Basically just dull the cutting edges a bit. I usually just drag the cutting edges over a fine stone or use a diamond file.

jim rozen · Oct 18, 2021

I advise against dubbing the edge on a 1/16 drill going into copper.

52 Ford · Oct 18, 2021

jim rozen said:
I advise against dubbing the edge on a 1/16 drill going into copper.

Ehhhhh... I think it's worth a shot. Especially since they're doing this on a CNC machine. More torque on the drill bit, but it aught to be less "grabby".

Could also try peck drilling.

Maybe use a sharp drill and go at a more conservative feed rate?

mike44 · Oct 18, 2021

My grandfather turned a good amount of copper and he used straight flute drills. At first I thought they were reamers. He also used milk instead of a cutting oil.
Not sure if these drills are available today. I dub the cutting edge and also the flutes on one set of drills. I mark these drills with blue dykom on the shaft so I do not mix them up with other drills.

mnl · Oct 19, 2021

Back in the day we machined a lot of OHFC copper. Holes were typically much smaller, ~0.020”. No attempt was made to dub them. Drilling was always done by hand with a sensitive drill chuck. The only lubricant used for copper was lard oil.

jim rozen · Oct 19, 2021

mnl said:
Back in the day we machined a lot of OHFC copper. Holes were typically much smaller, ~0.020”. No attempt was made to dub them. Drilling was always done by hand with a sensitive drill chuck. The only lubricant used for copper was lard oil.

Our standard lube for copper is 50/50 kerosene/lard oil. Dead sharp drills. The drill breakage mentioned is probably because of low spindle speed and excess feed rate per turn.

boslab · Oct 19, 2021

We used tallow in work, came in big sticks for Ali saws
Had a funny thought, we used a big pacemaker lathe to machine copper Lance tips, like 25’ centres, I was imagining cleaning the drip dray from swarf flavoured yogurt, not nice
Electrical copper was a pig, beryllium copper was fairly tolerable
Mark

doug925 · Oct 19, 2021

Emilyfinchum said:
Hello everyone. Needing some help with drilling a .062 hole into .130 diameter material on a lathe. My current program reads as follows
G97 s1000 m13;
M98p1;
T4x0.;
Z.2 s3000;
G1 g99 z-.65 f.0005;
M98p1;
I'm running on an older hardinge lathe, with barely any stock protruding from the face of the spindle and it pulls out to part length after it drills to prevent the stock from bending. Chuck pressure is all the way down to 30psi to prevent crushing. Carbide through coolant drill.
I've managed to make 1 part and the drill broke on the second. I've tried many different speed and feed combinations with no consistent luck. Does anyone have any ideas what to do to get this thing to run consistent? Thanks in advance

I just finished drilling 0.039" holes through 1" of 99% pure copper.
The drill was a standard, jobbers drill. Nothing specialized for copper or anything.
I broke the first drill trying to do it manually.
Then I changed to the cnc mill, flooded the drill with coolant, & pecked it out.

S8000M3
M8
G00 G43 Hhh
X.xx Y.yy
Z.zz
G83 X.xx Y.yy Z.zz F0.0008 Q0.01
G80

It worked beautifully, and ran with no problems.

Doug.

Advice for drilling solid copper

Plastic

Titanium

Diamond

Plastic

Plastic

Diamond

Diamond

Diamond

Plastic

Stainless

Stainless

Stainless

Diamond

Stainless

Aluminum

Hot Rolled

Diamond

Titanium

Titanium

Similar threads