Milling copper

[Burn]

Hi Guys,

I am probably a ways off from making chips, but I wanted to get your opinions on end mills for machining copper.

Specs:

• Max 3/8" cutter (Taig CNC w/ ER16 spindle)
• 2 or 4 flute?
• The Taig is able to go up to 10,000 RPM
• I will probably be going into the copper at max probably around a half-inch.

Any links to endmills are appreciated. Preferable from Enco or MSC

Thanks guys!

[dertsap]

standard 2 flt carb em should be sufficient for copper , if you don t have ample coolant i would suggest not running the tool at too high of an rpm to avoid a melt down

[Burn]

Thanks

I think I will have a flood setup in the near future- It does not sound that hard to do...In the meantime, if I run a 5 IPM feedrate would you suggest I run it around 750 RPM if I use, say, a spray bottle?

[Steve@Reliance]

Chip evacuation will be your biggest problem, followed by peventing a built up edge on the cutter. Use fluid with as much lubricity as possible. Copper conducts heat well so heat will be less of a problem. Keep your tooling dead sharp and use rigid setups because the stuff grabs. always climb mill to keep chips from sticking to the part.

[Burn]

Thanks for the tips

[Rustybolt]

If it's dead soft copper don't even bother without coolant. It's very important to carry the heat away from this type of copper. Use a lot of coolant. Run your cutter fast and use light feeds. Otherwise in a slot or a hole the copper will want to grab the endmill.

[Burn]

I was thinking of the halo-type coolant lines from LocLine, the ones that go around the spindle/bit- I think that type of setup would be best, right?

[Rustybolt]

Sounds good. Anything that will flood the tool with coolant. If you are going to tap a hole in copper shoot for 75% threads.

[Paul_S]

My best guess-estimate would be using a HSS 2 flute 3/8 cutter 200 sfpm or 2040 RPM with a chip load about .0017 IPT that is, 6.8 IPM. A carbide cutter the same size and depth of cut 7280 RPM with a feed of 12.8 IPM, that's .0009 IPT. Assuming the horsepower at the spindle at 2hp. If your spindle has over 3hp the the feed can be 15.8 IPM, that is .0011 IPT.

[Bud Guitrau]

Don't know what grade of copper you are milling, but Rusty is correct, you must manage heat build-up or the chips will quickly weld to the cutter and ruin your finish and size. Use dead-sharp end mills and always climb-cut copper to prevent pushing a burr on the off-edges.

[ran2]

Form taps work great in copper and make a stronger thread. Also if its just a few parts, HSS tooling and WD40 will get you by nicely.

[Burn]

Sorry to bump this but I have to start ordering endmills for this project. So the consensus is HSS, should I purchase anything with a coating on it? I am going to be buying 3/8" shank endmills so that I can run it with a 3/8" collet. Two flute or three flutes? I am on McMaster right now looking for them.

Got my 1/2" loc-line kit in today