Help! Noob broke so many EndMills, the store ran out

[Frogblender]

Breaking alot of bits here

Shown in the picture is a 4-flt .375" endmill .050" DOC, 5kRPM, 10IPM, spiral climbcutting a 1" hole in 6061. Strong air jet blows chips. But every once in a while, a melted glob of aluminum gets welded to the cutting edge (as shown in the picture), and the fun begins. I can tell when this happens from the noise, and hit the E-stop.

What am I doing wrong? Any help would be greatly appreciated.


I've broken alot of 4-flute 1/8" bits for the same reason , although I haven't broken a 3/8" yet....

[khbash]

Hi there, I would try some coolant/cutting fluid on it to stop the chips building on the cutting edge. I found dry milling difficult with chip build up. some coolant spray will most likely help.

[dneisler]

On my X3 using 6061 Alum, 3/8" bit and 5-6k rpm I cut at 24-40 IPM. The faster you cut the more heat you would remove with the swarf.

[Cruiser]

Use two flute with mist or flood (mist = liquid coolant syphoning into air blast !)
increase feed

[digisnapmark]

In my shop, I find that a single flute tool "0-flute" works best... 2 flute 3 flute, 4 flute all clog up much more often. I use a micro-drop coolant as well, and I think some sort of lubricant / coolant is essential for 6061....

[davereagan]

5000 rpm dry is crazy. If all you can do is brush tapmagic on by hand, I'd run more like 2000 rpm. Higher helix endmills specifically made for cutting aluminum make a big difference.

[mc-motorsports]

2 flute endmills for sure.

Is the EM in the pic TIN coated? If it's TiN coated, that's most of your problem.

Read through this whole thread:
http://www.cnczone.com/forums/showthread.php?t=83609

MC

[LeeWay]

You can also take much lighter cuts and really increase those feeds. 6061 isn't as prone to gumming up as some other aluminums. 5052 is very bad at this. I won't even mill it much anymore. I cut 6061 all the time at 6600 RPM, .01" DOC and feed @ 40 to 80 IPM. This is with coolant though and using 1/8" and 1/4" end mills. 3 flutes on the 1/8". 2 on the 1/4".

I rarely break an 1/8" em. Once a month maybe and haven't yet broken 1/4" after a year and a half. In that time, I have made thousands of these parts. They are the best ratio on parts per tool cost that I have. In steel, I get from 12 to 20 of those parts per tool. Not nearly as good.

I am starting to get even better results in steel with US made carbides though. First ventures into carbides were not so elegant. Mostly my fault by not knowing how to run them, but the machine is better tuned now as well. That makes a big difference with carbides and cobalts.

[Caprirs]

Originally Posted by mc-motorsports 2 flute endmills for sure. Is the EM in the pic TIN coated? If it's TiN coated, that's most of your problem. Read through this whole thread: http://www.cnczone.com/forums/showthread.php?t=83609 MC

I would agree with the TiN coating being bad for dry machining of aluminum. An uncoated tool with polished flutes/inserts would be best for aluminum.

A couple other points. First, 5000rpm is pretty slow. One aspect of the "dry" machining trick is to get the spindle speed high enough to eject the chips up the flutes and away from the cut zone. The coolant or air blast is to clear the chips primarily. Cooling the tool bit is secondary. I have a 1" two flute insert tool that I run at 8500rpm. 1" @ 8500rpm = 2225 sfpm compared to 3/8" @ 5000rpm = 490 sfpm. If I could run 12Krpm on my machine, I would.

The second point is I can buy a lot of endmills for the cost of repairing my air compressor. Whenever I have tried the dry machining/air blast, my compressor runs 100% and sometimes gets hot enough to trip the thermal overload on the motor if the job is long enough. A screw compressor wouldn't care but the piston compressors are rated in hours of life.

Running a 2 or 3 flute tool would also benefit by giving more space for the chips to clear.