On 04/13/2017 09:41 AM, Todd Zuercher wrote: > Here I go again. Unfortunately, the aluminum jig was a big hit, and now they > want more. So I thought I'd take a crack at a trochoirdal milling path. My > first try gave mixed results. Looking for advice. > My CAM software still doesn't have a trochoirdal option, so a faked it with a > line of small circles strung together. > I tried milling with a Vortex 1230 1/4" solid carbide up spiral @ 18000rpm > feed rate set to 100ipm (but due to machine acceleration limits the feed was > really only 60ipm). The path was made with 3/8" circles with a female climb > milling path strung together with a 0.05" step, milling 1/4" deep. It cut > beautifully, for about an inch, then the flutes clogged and the bit promptly > broke. This was a dry test cut in the Mic-6 chewing gum and I forgot to turn > on the air blast. > > Suggestions on where I should go from here? Smaller step? Lower or higher > RPM? Larger circle (to allow faster feed)? I know Getting the air blast > turned on and a squirt of WD-40 will help, but will that be enough? Better > Aluminum stock should also help, I have 3 sheets of 6061 for the next ones, > but I would like to cut a few things from the Mic-6 scrap left over from the > last one. > Well, either air blast or flood coolant (maybe even mist would work.) 18000 RPM and 60 IPM feed means .0017" feed per tooth on a 2-flute cutter, or .0008" on a 4-flute. That seems awfully small. If you are running as fast as your XY can feed, then I'd reduce RPM by at least 2X and stay at the same feed. My rule of thumb is to step down in Z equal to 1/2 the tool diameter. I think you could increase the side step to maybe twice what you were doing, .1"
So, you are cutting out the whole interior of the part? It might make sense to drill the center out with a lowly drill bit, then mill the final profile. The worst thing in the world is "plowing" an end mill at full width through the stock, ie. starting at the center and then spiraling your way out. That first turn is the worst. WD-40 is pretty awful, but may be better than dry in gummy materials. The whole trick it to prevent the work from heating. Aluminum goes from gummy to sticky mush at temperatures you can hold in your hand! So, the only help is coolant or taking extremely light cuts at high feed rates to keep the heat production moving along the work. 6061 is better, but you still have to keep it from getting warm. Jon ------------------------------------------------------------------------------ Check out the vibrant tech community on one of the world's most engaging tech sites, Slashdot.org! http://sdm.link/slashdot _______________________________________________ Emc-users mailing list Emc-users@lists.sourceforge.net https://lists.sourceforge.net/lists/listinfo/emc-users
