Save my sanity - 1050 grade aluminium

I need to cut some brackets out of 2mm and 3mm aluminium and have ended up with 1050 grade but its terrible. As soon as I started cutting there was just lots of noise and very little cutting, it just pushed it out of the way and clogged the cutter. Now after multiple speed/feed tests I still haven't made a single chip and I'm ready to break out the scissors :wink:

Any ideas, I have cut 5083 before and even when I messed up the settings that would cut fine. This stuff is shite but its thin enough for what I need and I already have it. :)

-I

Just dug out some 5083 that I normally cut at 0.4mm doc 800mm/m 15krpm. I took Jazzcnc advice about pushing it to see what your machine can handle and with a 6mm carbide(2 flute, 22k rpm and 800mm/m I have reached 1.5mm doc and it looks clean. I could probably push it a little more but I was getting sprayed with hot aluminium chips. It actually sounded better with the deeper doc.

Too bad the 1050 isn't 5083 :(

I was going to say, aren't the 1000 grade pure aluminium and is like trying to cut butter, in the fact it'll just move and clog everything?

Use a small single flute cutter, like 1/8th.

I've been cutting a lot of sheet alu lately and they're really great.

Quote:

---

Originally Posted by Isaac

I could probably push it a little more but I was getting sprayed with hot aluminium chips. It actually sounded better with the deeper doc.

---

Then your cutting something like correct because you want the heat to leave with the chips and not stay in the material or cutter. That said 22K and only 800mm/min is a little fast and slow. You could try lowering the Spindle speed a little to around 15K or up the feed rate.

1050 is a pain in the Arse and I don't cut enough so still haven't found the balance but I've had most success with twin flute slot cutters and cut full depth in 2.5mm sheet.

I've ordered some 3mm single flute cutters, but I have never used a cutter that small on aluminium. How do I adjust speeds/feeds to match? Half of what I use for 6mm?

From a popular F&S calculator tweaked for my machine (see my build log) in 1060 (no 1050 option sorry) I am getting 19,268 RPM and 684 mm/min using a single flute 6mm carbide cutter (20mm stick out) slotting at 2mm DOC.

I had some 3mm aluminium sheet, which I had before moving onto 6082 and likely to be 10x0 grade that cut OK using the above.

Softer stuff is a pain though.

5083 H112 (a softer variant) is coming up with 17,193RPM and 610mm/min with the other parameters above the same.

I cut some parts from 1050 the other week. Yes, it's a bit of a devil to cut but I found the slower the better... These are the parts I cut:

Attachment 12462

And here's a clip of the machine at work. (Yes, that is the alu sheet bending while getting spot drilled - I was feeling my way around the RPMs needed...)

https://www.youtube.com/watch?v=pFW-WvpHMQg

And here are some cutting details - all very conservative:

Spot drill - 10k RPM
HSS Through Drill - 5k RPM
3mm 2 Flute Carbide Cutter - 10k RPM
1mm 2 Flute Carbide Cutter - 13k RPM
Plunge rates at around 0.75-1mm/sec
Feed rates no higher than 3.5mm/sec

WD40 - a must. The cutter squeals a bit without it...

Wal.

Nice parts and vid - subscribed :-)

Also that's a good collection of bass guitars on your channel - I've been toying with the idea of cutting a new neck for my strat on my machine.

Cheers


Chris

Cheers Chris.

Hehe, I got into the whole CNC thing because of wanting to build my own bass. So far I've built the machine that'll help me build the machine that builds the bass..!

I could really do with getting rid of some of my (ahem... 11...) basses - but there's an excuse for keeping every one of 'em.

Would love to see your progress should you decide to make the neck - a worthy challenge for sure!

Wal.

Quote:

---

Originally Posted by Wal

I cut some parts from 1050 the other week. Yes, it's a bit of a devil to cut but I found the slower the better... These are the parts I cut:

Attachment 12462

And here's a clip of the machine at work. (Yes, that is the alu sheet bending while getting spot drilled - I was feeling my way around the RPMs needed...)

https://www.youtube.com/watch?v=pFW-WvpHMQg

And here are some cutting details - all very conservative:

Spot drill - 10k RPM
HSS Through Drill - 5k RPM
3mm 2 Flute Carbide Cutter - 10k RPM
1mm 2 Flute Carbide Cutter - 13k RPM
Plunge rates at around 0.75-1mm/sec
Feed rates no higher than 3.5mm/sec

WD40 - a must. The cutter squeals a bit without it...

Wal.

---

I'm getting somewhere now!

I dropped to 13k, 600mm/minute 0.75DOC with a 3mm single flute carbide and I'm getting a clean cut with fairly big C shaped swarf. It brought a tear to my eye ;)

Cheers guys!

Quote:

---

Originally Posted by Isaac

I'm getting a clean cut with fairly big C shaped swarf. It brought a tear to my eye ;)

---

Ooo - safety goggles..!

Hehe, glad to hear that you've hit upon numbers that are working for you. Well done.

Wal.

Cutting ali is better with an open flute, like these, which I use.
Sorotec - Werkzeuge

Moderate feed rates and spindle speeds give good results (even on my MD machine :ambivalence:) with a little bit of air to clear the chips and a drop of paraffin to cool and lubricate the cutter.