drilling copper - oversized holes

[Bob W.]

When I drill copper (110) the holes come out several thousandths oversized. What is the secret to getting accurate holes with this stuff? I am using a .128" HSS drill so speeds and feed recommendations would be a big help.

 

Thanks,

Bob

[gcode]

I would try a 135 degree spit point premium cobalt

drill.

If you are doing lots of holes for a production job, look into high performace solid carbide drills from Ghuring, OSG etc

[connormac]

I've also had a lot of luck using G73 for chip break. Then you can crank the feed up. Makes a better hole because the tool isn't re-entering the soft material so much. Use lots of coolant.

[horsepowered]

I use 3 flute solid carbide drills Tin coated from guhring with great success. Lower speeds moderate feeds and as ConnorMAc said chip break toolpath for deep holes.

[Guest]

The whole thing with copper what ever tool you use, is a sharp tool and a not overly aggresive feedrate as copper is very soft and will bulge and tear. ConnerMacs suggestion is a pretty good one, break the chip but keeps the tool engaged within the material.

[Greg Williams]

use a sharp uncoated carbide drill

[Tim Johnson]

Also if you're center drilling, use a No.1 cd and drill it .050 deep max. Copper has a tendency to grab a drill and pull it offcenter creating an oversized hole so you want to either use a split point stub hss drill, a split point carbide, or make the starting hole just barely bigger than the web.

[Jim at Gentex]

All good suggestions and advice.

 

Remember though, a twist drill is not designed to be a close tolerance cutting tool!

 

I know it requires an extra op but if I need a tight tolerance hole in copper I always drill it undersize then ream it to finished size.

[88Matt]

How deep is the hole? Through or blind? Many a good suggestion listed. I like Tim & Jim's suggestions, especially for deep holes in copper with tight tolerances. What is your tolerance anyway?

 

If they are shallow, try helix boring using carbide CB EMs. Once dialed in they would be faster than drilling and reaming. Just a thought.

 

Matt

[Bob W.]

Yeah, I always ream tight tolerance holes and I usually figure drilled holes to come out +.001-.002 over the nominal which is fine in this instance. These were coming out +.006 or so, which was much more than expected. I was also using a .125" carbide spotting drill to prevent wanter.

 

The holes were .25" deep and they were blind.

 

I'm curious more for future reference than anything because even at .006 these will work. I didn't know if there was a rule of thumb for drilling copper to get reasonable hole sizes or not.

 

Thanks for the help.

 

Bob

[Nick_AFRL]

We cut alot of oxyfree copper here at the lab, i would say about 80 percent of out work. The rocket nerds like it for its heat properties. When ever there is a call out for a percise hole, we center drill so that the countersink is equal to the dia of the margins on the drill. Then drill under size and use a reamer....

[Tim Johnson]

quote:

---

I was also using a .125" carbide spotting drill to prevent wanter.

---

If the spotter is 120 degree the drill shouldn't pull (though it may want to wander if the drill is sticking out far enough). If it's less than 120 degree then you might want to make sure to keep the dia barely larger than the drill chisel point.

[Kevangel]

its kind of basic, but a less than perfect sharpening job will make a drill drill oversize and crooked. Even a (bad) new drill will do this, some of the cheapo forgien jobs are bad to start,saw some once from China with the relief ground backwards on the point.I only buy usa after that..