[beeman_mccheyne]

Hey There,

I have an AXYZ 4x8' router table, 10hp spindle and am trying to work on my first real aluminium project - making profile cuts on letters around 18" high and some other pieces.

I did a test run - a small piece (2.5"X6") with some engraving and it turned out pretty bad. I mounted the 5052 .25" alu sheet on the vacuum table and secured it with some set screws just in case (into the mdf) and proceeded to cut out my piece.

Issues on the engraving (1/16" depth) - the edges weren't clean at all.. lots of burrs and the bottom finish felt grooved. I used a 1/8" 2fl upshear carbide end mill for the engraving with 15ipm@9100rpm.

Issues on the profile cut (.25" depth) - The piece started to move about half way through. I used a rod to hold it down while the machine finished up the job. But again (before the hard vibration) the cut wasn't super clean and left burring on the face. I was running a 1/4" 2fl upshear carbide end mill for the profile cut, 20ipm @9100rpm.

I hear stories of shops that can rip through this stuff pretty quickly and get good results, so I was wondering if anyone can advise me on what to do. I know I can add bridging to stop the part from moving, but on a letter that would be 18" high, would that be something people would do? As for the cuts, I'm all ears on hearing what you guys run for bits and feeds and speeds, I heard one shop running 1/4" bit, 200ipm @ 10000rpm and am so confused as to why I can't get a good cut at what I had programmed in. Both bits I used were brand new.

Cheers,

Frazer

[Med-Pac]

I'd recommend a harder alloy. We have cut some 5052, but a majority of our pcs are 6061, 7075. Lighten up on your depth of cut for everything, and slow down the spindle. Especially the engraving. Flood the part with coolant, and be ready to babysit the machine (with a bottle of WD-40), while you're cutting.

Hope that helps ya,
Mike

[Bob La Londe]

I had some left over 5052 from marine projects when I started machining. I found it machined like crap. Tended to tear and smear rather than cut. I almost gave up on aluminum before I discovered how much easier 6061 machines.

Anyway, sharp, fresh cutters...

Flood coolant

or

Air blast to clear chips, and a few drops of Tap Magic for aluminum rubbed on the stock may help.

[JohnZ]

While I do not have a ton of experience with aluminum, the following worked for me machining some 5052 1/4" thick sheet that I picked up from the scrap yard.

45 ipm
.020" depth of cut
10,000 rpm

With other types of aluminum I can go with a higher rpm and a deeper depth of cut. But with the 5052, I had to take it easy. I also had to keep the chips constantly cleared out with a blast of compressed air and spray some wd40 to keep the bit from gumming up. If you can go with a faster cutting speed, that should help a bit too. If my router could go slower, I could probably make a deeper cut at a slower ipm and maintain the same material removal rate. Once I get my new spindle finished (0-5k rpm), I'll be able to do some additional testing.

Sent from my DROID4 using Tapatalk 2

[Boltz]

I've gotten best results cutting aluminum with a single flute bit which has a mirror-like polish in the gullet. One example is the Onsrud super "O" bit.

The 2 flute endmill not only has 2 edges rubbing in the cut generating heat, it also has a flat end, which is rubbing on the bottom of the cut and also generating heat.

I'd also recommend taking shallower cuts and moving faster. I like to be moving at least 1 IPS in AL.

-Jim Hart

[beeman_mccheyne]

Thank guys! It was a little bit of an older post, but I did find a solution in the end. I did pick up some single flute "O" upshear bits and they seemed to perform much much better than what I was getting with the 2 flt. I also bought some cutting fluid and built an air blaster. I probably should post my speeds and feeds.. will do when I get back to my log book.

Thanks again!

[nickm87]

I would have suggested what you have now done but glad you got it sorted. Look forward to hearing about your feeds and speeds.

[ftptorrent]

One last thing.....if you're using toolpath, make sure in the Output menu you have REVERSE under Machining Path and not FORWARD. Good luck.

[daytona81]

I realize this an old post. Been working with 5052 for about a year now. Use wd40 as a lube. i promise its a miracle worker. if you dont have a mister just spray an even coat. Also, try an onsrud single flute. i run full depth cuts on .100 5052 35ipm at 12500rpm.

[aarggh]

I realize this an old post. Been working with 5052 for about a year now. Use wd40 as a lube. i promise its a miracle worker. if you dont have a mister just spray an even coat. Also, try an onsrud single flute. i run full depth cuts on .100 5052 35ipm at 12500rpm.

WD40 does work fantastic on cutting aluminium, but as it's a fairly noxious chemical brew, I use lanolin based lubes instead, works just as well, but no dangerous fumes or chemicals.

cheers, Ian

[underthetire]

Olive oil works great as well.