[Kingjamez]

I just snapped a brand new end mill and I can't figure out what I did wrong. I was doing a .1" DOC @ 14 IPM cut on my X3 with a 3 flute 1/4" HSS coated end mill from Enco. I plunged into the metal at a rate of .1" in 2" and it was sounding very smooth. After the plunge was complete it started a full width slot at 14 IPM. It still sounded very smooth and then just SNAP, broke right below the collet.

Anything above look suspect? I would like to have some "reason" before I load up another end mill. I'm about 3/4 of the way through a job and really don't want to screw the already completed work up.

-Jim

[ckirchen]

What are you cutting and what are you using as coolant?

[Kingjamez]

Right... that's important. I was cutting 6061 and using KoolMist #77 from a spray bottle.

-Jim

[ckirchen]

Sounds like the flutes packed up with aluminum, which then limited its ability to cut, and snapped due to the oncoming material.

Aluminum has a very high tendancy to bond to the cutter if the cutter gets hot. You need better cooling, which is why I always use flood coolant with aluminum. If I forget to turn the nozzles on, the same thing will happen.

Do you have flood coolant available?

If not, you could try a lighter DOC. In a pinch, I've been know to use a .005" to .01" DOC, aim an air nozzle at the cutter, and turn the feed rate way up. The goal is to keep the cutter cool.

[Kingjamez]

I checked the end of the mill for welded aluminum chips. It was clear and sharp.

I can flood, but I can't catch the coolant. I don't have an enclosure. So misting will have to suffice. I just got done hogging out the aluminum with a 1 flute .5" end mill and that worked just fine with the mist.

-Jim

[SCzEngrgGroup]

This may sound crazy, but you probably want to feed faster. How fast depends on your spindle RPM. You should probably be running yor spindle as fast as you can (I'm assuming you're limited to 2K-4KRPM). Then calculate feedrate based on a chipload of perhaps 0.003-0.004"/tooth. Start with a shallower cut, at a faster feed (20-25 IPM should probably work), then go deeper until it starts having trouble. When you get it right, the chips should be coming of VERY hot, the tool should remain quite cool, and the tool should be making a nice, constant, kinda cool, whirring sound. Also, make very sure the coolant/air is flowing strong enough to blow all the chips out of the cut.

At 1/4", you'd likely be better off with a 2-flute for slotting. A 3-flute that small will not have a lot of room for chips to escape. It only takes a momentary clog to break the tool.

Regards,
Ray L.

[Kingjamez]

Hmm... to be honest that does sound crazy. :-) It seems to me that the correct chip load is the correct chipload at .05 DOC or .1 DOC so I don't get the recommendation to increase my speed.

I did reduce my DOC and ran the program again and it worked great. No flood needed, just a little mist and a good feed rate.

-Jim

[SCzEngrgGroup]

Hmm... to be honest that does sound crazy. :-) It seems to me that the correct chip load is the correct chipload at .05 DOC or .1 DOC so I don't get the recommendation to increase my speed.

I did reduce my DOC and ran the program again and it worked great. No flood needed, just a little mist and a good feed rate.

-Jim

"It seems to me that the correct chip load is the correct chipload at .05 DOC or .1 DOC" - Not necessarily true. It CAN be, but often is not, for many reasons. It depends on the tool, the material, the cut, the coolant, etc. In general, the deeper you go, the more you have to slow down to avoid clogging. Also, for shallow cuts, chip thinning comes into play, which can require significantly increasing speed to maintain the same effective chipload (vs the apparent chipload). The slower you go, the more heat is likely to build up in the tool, so you want to go as fast as the tool will allow, so the chips carry the heat away. In general, if the tool is getting hot, you probably need to either reduce RPM, or increase feed (both of these increase chipload), or reduce DOC. Often, a combination of the above. For me, a common roughing cut in 6061 is a 1/2" 2-flute HSS endmill, 0.250" DOC, 3200 RPM, 30-35 IPM. Up to about 0.125" deep, I can do it with just air, no coolant, and the tool stays cool. But slow down to 15 IPM, and the tool will clog, jam, and break off in a few seconds.

There are aspects of speeds and feeds that are rather counter-intuitive, until you get the hang of it, and understand more about what's going on where the tool hits the work. It's a complicated area, and the answer is different for every combination of tool, material, machine and cut.

Regards,
Ray L.