Page 2 of 2

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 12:17 am
by TomDChi
jbc wrote:How would you rank cam programs for a beginner?
I know of meshcam.
I'm a CAM beginner but not a CAD beginner. I've really been liking Fusion 360, particularly the "free for hobbyists" part!

The curved profile on the arms of your widget make me think that you'll be looking for something that does full "3D" CAM, and Fusion definitely covers that. But... I don't have a sense of how heavy a lift it is to learn as a beginner.

How big is that part overall? I think the big difference between the SO3, where we're talking about doing stuff at 10 ipm versus bigger, more powerful systems is just the time it would take to mill those parts, once you have it all figured out.

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 3:54 pm
by JeromyReno
jbc wrote:How would you rank cam programs for a beginner?
I know of meshcam.
I use cambam for everything. it has great features if you are converting art into cam files and the ability to adjust and tweak every aspect of the operation. you get 40 free uses with it for a trial and that will pretty much last you forever haha. I am on use 11 and used it on dozens of projects, and I have been using it for a year, im so used to it now that I will no doubt be buying it when I stop spending money on other stuff for my machine.
I have used meshcam, I did a trial of it and it's as easy at it gets, you just enter a few things and away it goes. it seems very beginner oriented. the price and ability to adjust every parameter in cambam it what attracted me to it. I guess im just a cheap control freak.
TomDChi wrote:
Personally, I'd watch and probably learn from it! From all the standard stuff I've been reading about milling metal, I got the impression that you needed to be cutting chips of some minimum thickness, or else the cutting edge would just rub and heat up/soften the material without really cutting it. With the minimum RPM of the DW611 (16,000 rpm) and 10 inch per minute feed, you're well less than a 1 mil chip, which is much lower than anything I've seen recommended in manufacturers' feeds and speeds charts. But obviously, it's working!

Are you using a single flute end mill? Coated?

Regarding "coolant"/lubricant, what system/fluid are you using? Did you experiment at all with applying stuff as you go - i.e. spritzing a little WD40 or Tap Magic as things move along. Or did you go straight to a mist/spray system?


I have been using a 1/8 Dia. 1/4 Flute Length 1/8 Shank 1.5 OAL AlTiN coated center cutting bit for the last few weeks. before I was using a 1/8" Variable 2 Flute End Mill for Aluminum ZrN coated. it and a great chip evacuation but the over all finish of the part was similar. im using a trico air/oil spray, it's way over kill. it has two spray heads and I have one turned off. I also bought a 20$ one on ebay that would probably work just as well that I plan on trying out, you want the air to cool down the part and bit while evacuating the chips from the work piece, when your bit tries to cut threw chips in a piece it's like throwing a stick in bike spokes. it deflects the bit making it try and cut more than it can. I keep the cutter speed down around 2 with the 1/8 but.

i'll make some videos and put them on youtube if you guys are interested.

http://www.lakeshorecarbide.com/18carbi ... flute.aspx

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 4:00 pm
by TomDChi
I'd also love to see more videos of the Shapeoko 3 milling aluminum... so I made one:

https://www.youtube.com/watch?v=zg7k21xPB60

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...)

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 4:46 pm
by jbc
JeromyReno wrote:
I use cambam for everything. it has great features if you are converting art into cam files and the ability to adjust and tweak every aspect of the operation.
Have you used meshcam? I have not used either but like your comments about cadcam.
by TomDChi :
I set up the CAD and CAM in Fusion 360
I've done all of my dac with Sketchup which has worked well for my 3D printing needs.
I am trying out Fusion 360 and like their UI but of course no experience with this and a CNC machine.
Anyone else using Fusion 360 and have found a solution to the missing 'J' values?

And TomDChi, thanks for the video!

jbc

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 4:50 pm
by JeromyReno
I usually do a rough cut first at 10 ipm that leaves .005 and come back and do a full depth path that cleans it off and a much slower speed, 3~5 ipm

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 6:28 pm
by TomDChi
There's ongoing discussion of the Fusion 360/grbl post processing here:

http://www.shapeoko.com/forum/viewtopic.php?f=16&t=6328

I should clarify - this may not be a problem between Fusion 360, the grbl post processor and grbl running on the Carbide control board. It may only be Carbide Motion objecting to the missing values. I haven't made time to test if grbl accepts the g code as-is out of Fusion with the generic grbl post processor. (Too anxious to just cut stuff with the time I have available in front of the SO3!)

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 6:31 pm
by TomDChi
JeromyReno wrote:I usually do a rough cut first at 10 ipm that leaves .005 and come back and do a full depth path that cleans it off and a much slower speed, 3~5 ipm
In the lead up to actually getting the machine, I kept reading and hearing "don't baby the cut!", "too slow a feed and you'll just skim the surface and heat harden it!" and so on. Now that I'm actually making cuts... I'll happily try your approach!

Are you using straight carbide or something with a coating?

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 7:41 pm
by WillAdams
TomDChi wrote:I kept reading and hearing "don't baby the cut!", "too slow a feed and you'll just skim the surface and heat harden it!" and so on.
That's probably from machinists running much heavier, far more rigid machines.

Re: 1/4" Aluminum

Posted: Wed Aug 26, 2015 11:55 pm
by JeromyReno
TomDChi wrote:
JeromyReno wrote:I usually do a rough cut first at 10 ipm that leaves .005 and come back and do a full depth path that cleans it off and a much slower speed, 3~5 ipm
In the lead up to actually getting the machine, I kept reading and hearing "don't baby the cut!", "too slow a feed and you'll just skim the surface and heat harden it!" and so on. Now that I'm actually making cuts... I'll happily try your approach!

Are you using straight carbide or something with a coating?
I have used both ZrN and AlTiN and gotten the same results. I used to run a bridge port mill and I fully understand the problem with babying the cut. you where always riding the line between breaking a bit and heating the piece. but i feel like the bit can not remove enough material to carry away the heat. especially with a 1/8" bit. when i ran a 1/4 inch bit i was throwing burning hot chips and the part didn't even get hot unless i was doing long profile cuts so i was getting friction all around the bit. but everything i have been making requires small mounting screw holes and large profile cuts. the air cooling was the game changer. the oil helped on the profile cuts too.