Lube is your friend. I try not to do any aluminum cutting without lubrication. I think your air blast and lube will get you a long way towards better tool life.
What is the overall thickness you are cutting? If it is more than 1/4" I would recommend using the full cutting length of the cutter and taking a cut that is .1 times the cutter diameter. Calculate your feed rate based off that to keep tool deflection under 0.001". This will optimize overall tool wear and will improve productivity if you can keep the feed rate up enough. I am not sure that going to a larger diameter circle will help you any. It will increase the feed rate but it will also increase the path length probably not yielding a better run time. If the 60ipm is the best you can do slow down the RPM so you are taking at least a 0.001" per tooth chipload and are not rubbing creating extra heat that will increase the likelihood of chip weld. My 2 cents. Also as Andy stated Fusion 360 can be had for free or cheap so I would try that for these types of tool paths. Jim On 4/13/2017 9:41 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. > > > ----- Original Message ----- > From: "Jon Elson" <el...@pico-systems.com> > To: "Enhanced Machine Controller (EMC)" <emc-users@lists.sourceforge.net> > Sent: Thursday, February 23, 2017 12:54:14 PM > Subject: Re: [Emc-users] Milling Aluminum. > > On 02/23/2017 09:35 AM, Jim Craig wrote: >> Yep, you should have done a HSM slot about 3/8" wide with the 1/4" >> cutter and you would have had little trouble. I try to avoid a >> conventional full width slot in aluminum where possible. lube definitely >> helps or is required. >> >> > Yes, the hardest part of this is what I call the "plowing > cut", where the cutter is cutting the full width into the > material. There's no great way to do this, but ramping down > helps, some. There might be some inventive ways to ramp > several times down the cut, then make a pass at constant > depth taking off the tops of the ramps, then repeat at next > depth, etc. > until you break through. > > I never cut slots the same width as the cutter, I always > somehow manage to plow the first, full-width cut, and then > climb mill the sides to bring the slot to the desired dimension. > > 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 > > ------------------------------------------------------------------------------ > 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 > ------------------------------------------------------------------------------ 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
