I'd also love to see more videos of the Shapeoko 3 milling aluminum... so I made one:
My first try a few days ago was a mess. I picked up a few bucks worth of scrap aluminum a while ago, and no one knew what type/alloy it was. But, hey, my SO3 is reasonably set up, I'll put a basic 3/16" 2-flute upcut carbide end mill in it and try to cut a circular pocket... Well, my clamping wasn't adequate, and whatever feed rate I used was too much for that setup/mill/material, so it shifted around. But watching the video, right from the start, the aluminum was mushing out around the edges. The mill came out of this with some aluminum stuck to the flutes. Overall a mess.
Since then, I've put some t nuts into the base MDF on a 100mm grid, so I was able to bolt down my 3" vise. I don't have a lot of vertical working space because the vise is tall relative to the SO3's Z travel, but it's enough to try putting some holes in a bit of 6061 1/4" (0.26"/6.6mm actual) plate I got recently.
I'm using a 1/4", 2-flute ZrN coated end mill from Lakeshore Carbide (#320014X)
I've signed up for the 30 day trial of G Wizard, so I used that to get the feeds and speeds. I used an el cheapo "photo" tachometer to check the rpm setting on the DW611, at least under no load.
I set up the CAD and CAM in Fusion 360 to make a 0.5" diameter hole in a 0.25" plate. I set the feeds in Fusion roughly based on G Wizard's results - 11ipm (280mm/m) for the plunge/ramp and 20ipm (508 mm/m) for the horizontal feed. (This is down about 10% from G Wizard's recommended 23imp.)
The first cut went pretty well. I was surprised by how much the chips were really thrown while cutting, and the kick from 11ipm to 20ipm was a little startling, but it appeared to work well enough. I couldn't really see down into the pocket, but it did seem that the chips were being cleared reasonably well to avoid re-cutting. My only problem was that I had intended to cut the 0.5"(12.7mm) hole all the way through the plate. I didn't set up the CAM to go past the bottom of the modeled plate, and I also hadn't actually measured it, so I set things up as though it was 0.25" thick based on its nominal 1/4" description. I modified the CAM settings to end up about 0.05" beyond the bottom of the modeled plate.
I moved the gantry about 0.75" away, and re-zeroed, then ran the new code. (I also set up some 'barriers' of scrap wood to block a lot of the thrown chips.) The result was what I was aiming for - a hole all the way through. On this run, I only put down a little WD40 at the start (which you can see in the view, slid off rather than pooling at all), and didn't add any during the cut. It didn't seem to make any difference. The only problem was that I forgot to record that run. So I re-zeroed off to the side, and re-ran the cut again, but with the camera rolling. Again, everything went well.
The resulting through holes are not perfectly round. They have some waviness to the sides, and it looks like it's consistent between the two holes - the same bumps in the same places going around the circle. I think, from watching the video, that the most likely culprit is flex. I may not have the SO3 tuned perfectly, but it's also possible that 20ipm in 1/4" steel is more than the SO3 can do without some distortion.
But... the code that usually comes out of Fusion 360 using their generic grbl post-processor usually has some "J" (sometimes "I" and rarely "K") values 'missing'. That may well be perfectly standard g code, but Carbide Motion won't load code where these are missing. One possibility is that the "J" values are repeating from the previous G2/G3 line, but I'm not sure. In order to get the code to run, I've been putting in "J0" where ever the "J" value is missing, and it runs. It's very possible that the "bumps" on the sides of the circles are where the helix ends and the g code moves the mill out from that center spiral to go around the perimeter, and that I've messed that up a bit by slapping in "J0" where it should be a slightly different non-zero value.
One way I could check this would be to leave on "stock to leave" so that I clear the overall hole as a roughing pass, then come back and do a separate finishing pass. If the g code for that finishing pass is short and simple, then I could experiment and compare "J0" substitutions versus replicating the "J" value from the previous line and see if that cleans up the "bumps". A thin finishing pass at a slower speed would also reduce the flexing forces put on the SO3's gantry, as long as I'm cutting and not just rubbing.
(I also keep saying that I need to use Chilipeppr and see if it objects to the g code with the "missing" "J" values, and if it will load it, throw it at the Carbide Control board to see if it runs it or barfs, or get Universal G Code Sender working and try it with that. But I'm having too much fun actually cutting stuff...)
All in all, though, I'm really impressed by what can be done. I'll be picking up a 1/8" ZrN coated end mill from Lakeshore to see if the smaller diameter can plough through AL like I suspect it can. I'm also interested to try a "O" style single-flute mill for aluminum to see if that's different/better/worse. I'm also all the more interested in making a dust/vac shroud, if for no other reason than to contain the spray of chips. (Which weren't really that bad, but I'm in a small shop, so any mess is a big hassle and my computer is fairly nearby, which I'd like to keep entirely free from metal particles...)