The higher chip load is a step in the right direction, but without lube it isn't enough. Bit broke after about 1.5" of cutting, but it's flutes weren't jammed full of welded swarf this time.
I switched to the O-flute bit, and that seems to be the ticket. Single flute @14000rpm and 80ipm. It is milling 1/8" deep pockets full depth happily with a conventional fill path with .0625" step over and minimal lube application. ----- Original Message ----- From: "Jim Craig" <jimcraig5...@windstream.net> To: "Enhanced Machine Controller (EMC)" <emc-users@lists.sourceforge.net> Sent: Thursday, April 13, 2017 12:33:40 PM Subject: Re: [Emc-users] Milling Aluminum. Yea I thought your recipe looked pretty good. I think the missing ingredients are lube and chip evacuation. My steps below are my basic guideline for setting up a cutter for aluminum with HSM paths. I have not broke a cutter while using those guidelines and flood coolant since I started using them. I may be conservative but I don't like breaking cutters. Good luck and keep us informed. On 4/13/2017 11:22 AM, Todd Zuercher wrote: > My material is only 1/4" thick, so more tool engagement is not an option. > > I ran a test with 1/2" circles (1/4" loops for the tool center) and the feed > rate increased to 80ipm. I also decreased the step to 0.025". The results > were about the same. > With the 80ipm @18000 and the 2 flute cutter isn't the chip load a little > over 0.002" already. > > Next, I'll try pulling back the RPM to get a higher chipload. Aiming for > about 0.005" this time so I'll run 8000rpm. > Then I'm going to try a single flute O-flute cutter (with a alight up cut). > > ----- Original Message ----- > From: "Jim Craig" <jimcraig5...@windstream.net> > To: "Enhanced Machine Controller (EMC)" <emc-users@lists.sourceforge.net> > Sent: Thursday, April 13, 2017 11:27:42 AM > Subject: Re: [Emc-users] Milling Aluminum. > > 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 > > ------------------------------------------------------------------------------ > 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
