[bowhunter]

anyone familiar with machining copper? whats the best way to drill the stuff need to drill a .875 hole thru a piece 7 inches long? having trouble breaking drills in half and spinning the part in the chuck? thanks for the help

[Bud Guitrau]

Bowhunter,

Keep the part COOL! Copper readily conducts heat and as you drill deeper, the part expands (from heat) and pinches the drill body and causes bad things to happen as you describe. I'd suggest:

1) Flood coolant of both the drill and the part.
2) Decrease feed-rate.
3) Peck-drill to break the chips and allow better coolant penetration.
4) Worst case workaround is to relieve the lands of the drill to reduce friction.

Hope this helps.

Bud

[Metalmog]

From what I remember, reduce the drill point angle by about 10 to 15 degrees and increase the clearance angles a few degrees. Sharp tools with a fine finish are important (less friction). This will result in a fair thickness chip curling out and prevent cloging. Turpintine or parrafin makes a good lubricant, else use lots of overly diluted soluble oil (or condensed milk - apparently it's the "miracle lube" for copper cutting . You should be quite aggressive with feed but need to keep the temp down to prevent binding.

[fizzissist]

Just got through drilling 7/8 holes through a 4" chunk of OFHC copper....yuck.

Like they're saying...slow it down...way down. Like 200-300rpm, or even less. Retract often, especially when getting deeper to keep the chips out of the hole and keep things cooler.
Lots of coolant...and get this, I use 1/2 +1/2 when tapping copper, and it works great. Throw what you don't use in your coffee. But since that would probably be really messy for what you're doing, just keep things as wet as you can.

Use a SHARP tool. Copper acts like a real abrasive on HSS, so don't be surprised if half way through it's looking dull.

Be extra careful when it comes time to break through the other side, as it can grab and things can come unglued. Put some drag on the spindle and slow your feed down for that.

Copper is a real PITA.

...btw...next step...72 8-32 helicoil tapped holes...with a plug tap in the part, along with a 2.5" bore through each side. How lucky could I get?

[riverrat]

whatcha drilling on, manual machine, cnc?
I agree on buds assesment its getting hot and pinching your drill.
Flood with lots of lube, keep it cool.
it really machines pretty easily, you might try slowing down
the rpm's, or go with a gundrill setup with a spraymist system.
drillmasters has a pretty affordable setup, if you have the quantity
to afford the investment.

[masterblaster]

definatly flatten the point on that drill or it will bite too deep. Bring it back to 140-130 at minimum. copper tends to be very stringy and will pull any 118 drill right in.you want to think of milling with a drill bit. Don't pre drill too large either go maybe 1/4 - 3/8 dia for that size or it will bite too fast on the .875

[awalters2]

Copper Does Not Dissipate Heat Very Well.the Heat Seems To Stay In The Part While Drilling.
I Have Had Lots Of Succcess By Sharpening Only One Flute To Allow The Drill To Drill Slightly Oversize If Tolerance Is Allowed.this Will Allow The Drill To Rapid Back Into Hole Without A Press Fit Per Say.
If Necessary I Will Ream Holes.

[Servo Wizard]

bowhunter,

Step drill the hole: .500 dia drill / 1.00 deep and follow with .875 dia drill

[ewest]

The guys here say kerosene is a good lube (same as paraffin I saw cited up above), just don't fill your sump with it. My boss saw somebody do this once - nothing happened, but just imagine it....

I also agree that a stepped drilling approach would be good.

Andy

[jonkka]

Grind flats on the cutting edge of the drill bit. You should do that for any material softer than soft steel. Plastics, wood, soft metals.

You need to scrape your way through. Using a sharp edge like you use for steel will grab and try to pull it's way through very aggressively, but you've already seen that.

Depending on what you're cutting, you can do with a flat done by some a little time with a diamond hone all the way up to a little time on the grinder.

To be clear, make the cutting edge 90 degrees to the cut. I would guess about .015 inch back for copper. Start small. Try it. Make it more if needed.

[colemanimal]

ive had the best luck using solid carbide or carbide tipped drills and not pre-drilling at all; maybe a light spot, just enough to center the drill. ive done quite a bit of soft copper (C110) for parts (ie: buss bars and heat sinks) and hard copper for EDM electrodes using this method to drill holes up to 20 times diameter. ive found that the drill becomming dull in the hole is the biggest challenge to overcome. i believe the problems you are having are caused by the tip of the drill becoming smaller in diameter than the rest of the drill and the sides of the drill binding in the resultant tapered hole. best of luck.

@fizzissist, i would suggest using coated form taps for your multiple 8-32 hole pattern, if youve not already finished the job and if you would like somebody elses opinion. :stickpoke:
ive had the most consistant tapping results in soft copper using them, and you can spot wear by watching how much coating has been rubbed off.

[fizzissist]

Thanks for the thread former tip...but....Who makes helicoil thread formers? Granted, I didn't look maybe as hard as I should, but the readily available taps were not forming. That was actually my first choice.

One hint....from 1st hand experience...is that U-Drills in copper are NOT happy in the cnc.. It chattered like a big dog, and the resultant chips confirmed. Not to mention it woke up everybody in the shop.

I've broken the program up so I can double drill the holes, or re-drill with a second if the bottom gets tapered. I've got a serious depth issue, and tap breakage is not a good option.

[Bud Guitrau]

Grind flats on the cutting edge of the drill bit.

I agree with jonkka on this and I'm sorry I failed to mention this in my earlier post. When drilling copper (or any soft material, as jonkka has accurately pointed out), you should "lip" the corners of the drill. If you are skilled at offhand grinding, go to the tool & cutter grinder and carefully grind the "hook" away only from the cutting face at the corners of the drill, producing a small flat at zero degrees. This will allow the major cutting edges of the drill point to cut aggressively with a positive rake, but the small flats on the corner faces of the drill will prevent the "grabbing" a positive rake drill tends to do upon breakout in a soft material. To get a smoother finish and accurate hole size, you can also stone a small radius (.010-.015") on each corner, smoothing out any toolmarks sharp corners tend to leave.

Because of the diameter of your drill, you should also "gash" or "chiselpoint" the drillpoint, thinning or reducing the web thickness at centerline allowing it to cut instead of "pushing" at the centerline where SFPM is low. This will reduce some cutting pressure and the heat generated from it. Extra back clearance or relief behind the chiselpoint doesn't hurt either.

That's my 3 cents worth (<-- 2 cents, adjusted for inflation)

Bud

[colemanimal]

i dont know where to find the sti form tap off the top of my head, if theyre tough to find that is unfortunate.

tha carbide tipped drills i was referring to are single insert pointed or brazed, not the u-drill style. i suppose i should have been more specific.