Copper milling?

[jinu117]

Hello, I am trying to mill .3 inch deep 1/8 inch wide channel on copper block.
I've tried using 4 flute solid carbide bits and.... (killed quite a few of it).
I ran out of 1/8 I had in spare at this point and need to get some...
Before I run out and purchase more bits, I would like to get some idea of what I should really be doing
Max RPM of machine is 3500 RPM, cold air gun cooled (right after running some 3/8 cuts on copper, if I touch copper, it feels cold... probably around 10c or so)
There seems to be quite a few selection on endmill I could choose from (looking at mcmaster right now).
Number of flutes, type of material for endmill, and different Helix angle.
Also based on your recommedation, I would like to get some numbers at say RPM, depth and IPM... that I should be running this at.
Didn't realize copper was going to be this hard to cut with small sized endmill but I am left with not much choice at the moment.
Thanks in advance!

[tobyaxis]

Run your max rpm [3500] at 1.5 inches per minute taking .03 depths of cuts for each pass to start. Use a 3 flute carbide end mill and be sure to use the air blast to clear the chips. Also try to get TiN Coated tooling. If at all possible try to drill a line of holes about .093 in diameter and .125 apart.

Copper is gummy material so use quality sharp end mills like DuraMill, or OSG.

This are starting recommendations that may have to be increased or decreased.

[jjasshipley]

3500 rpm, .080 doc, 5.6 ipm - 3 flute carbide, if you go with a 2 flute slow your feed to 3.73 ipm. You don't want to use a 4 flute, the flutes will gum up to easily.

[JROM]

yes copper is gummy to cut but what really goofs you up is that as copper gets hot it grows! So as you are making a cut the copper right under the cut is getting hotter then the rest of it and poking up into the flutes at the BACK of the cutter. This will foul the cutter in a heartbeat and break it or ruin your part. If you can tip the head a couple of thou. so the front of the cutter is lower then the back. And point the cold air gun streight down on the cutter so the back is getting cooled as much as the front you will see a big improvement. Goodluck!

[jinu117]

Thanks guys, mixing some values among what you two have suggested...
I got to 3500 RPM, 0.03 doc 7.5 ipm (started at 3.5 to be safe) without much issues. Since I needed to cut few quickly I didn't progress much farther. It seems to work fine with the tool going in horizontal motion at the ipm but even with feed reduced to 1 ipm-1.5imp, it seems to make some more noise than I would like to hear (cuts fine still) when mill gets into the copper. I probably will try bit deeper doc with back to slower IPM progressively to see where it would be most productive slowly It would be fantastic if I can get 0.08 doc 5.6 ipm for sure as it will cut down time by more than half (with some g-code optimizations I will have to do once I am set on design).
I am using what McMaster carreis after some suggestion, wonder if anyone can comment on if OSG/Kenametals would be better... (It's from Niagara cutters, inc) and 45 degree helix with 3 flute and TiCN coated. It's supposed to handle heat better for non ferrous metal than Tin but I am wondering if it was even worth bothering as I found the cold air gun keeps both copper and bit below ambient temperature anyways...

PS) Just quick roughing cuts, etc on this. No need to make it finished really

PPS) woot. up to 0.06 doc 6ipm. Afraid to go any higher as I am noticing vibrations on table... -_-; I need to get better machine stand shortly if I want to go higher.