----- Original Message ----- > From: "Jon Elson" <el...@pico-systems.com> > To: "Enhanced Machine Controller (EMC)" <emc-users@lists.sourceforge.net> > Sent: Thursday, April 13, 2017 1:22:32 PM > Subject: Re: [Emc-users] Milling Aluminum. > > 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 >
But I'm cutting out a 2ft x 3ft window. It would be silly to pocket fill that entire thing. It seems I'm making good progress using the majic O-flute bit and a trochoidal path. ------------------------------------------------------------------------------ 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
