Cutting Shapes and letters from .040 Aluminum?

[Call-Tech]

Has anyone had any luck cutting clean shapes out of .040 Aluminum sheets. I have cut 1/4" aluminum just fine, but no matter what I do the .040 or .080 sign sheets just melt. I can cut half way through the .040 and it chips very nice, but as soon as it punches through and starts cutting on the side of the bit, it just melts.

I'm running pc and alpha96. Any recommendations for speed, bit type etc.. would be greatly appreciated.

[WCSC (Unregistered Guest)]

How small are your shapes and characters? It's going to be all about the hold down and bit size. 1/4" O bit i'll usually go 12,000RPM's @ 1 IPS 1/8" bit 18,000RPM @ .40 IPS. Also a lot will depend on the aluminum grade. Stay away from the 5k grade and use the 6k (forgot the alum numbers but you might know what i'm talking baout) the 5k series is softer and heats up more and will melt.

[Call-Tech]

Well the hold down is vacumn and the bit I was using was 1/4" at 10,000rpm and i tried .5 ips to 2 ips. This is just sign grade .040 aluminum panels available with color coat or plain. I'm sure that they are not t-6 or 6k aluminum. The pieces I am cutting are mostly letters or simple shapes about 6-8" in size.

I think the problem is in the type of cutter I am using. I am using one of the 1/4" endmills that came with my shopbot. I have not yet learned enough to purchase any others.

The aluminum cuts fine as long as I do not cut all the way through it. I can cut .010, .020, .030 without any problem, the aluminum only melts when I cut all the way through and it does not matter if it is the whole .040 or if it is just the last .005. When the cutter goes all the way through on the last pass or only pass if I make just one that it starts to melt. I can make a .035 cut and it cuts great, just chips and nice machined cut.

[WCSC (Unregistered Guest)]

I use Belin solid carbide single flute spiral O bits. 1/4 Bit I use the 33476 & 33635 1/4" bits and 33317 1/8" bit which fits in a 1/4" shaft. These bits work very good for me especially with aluminum. Hot knife thru butter best explains it. I have a mister which I haven't hooked up yet (collecting dust). So every 30 secs or so I spray WD40 in on the router bit as it's cutting and coat it with cutting lube prior to cutting. This will help keep it cool and longer tool bit life

http://belin-y.com

[signscad]

I use Hartlauer bit# 52-141h/ 1/8"Dia, 1/4" shank to route the .40 Brush Silver alum., sandwiched w/1/4" Acrylic,
double tape on blue foam and clamp to table.
My Vacuum System is Clamp and Double tape from Harbor Sales, for Dulles Airport Symbol 20" x 18" @10,000,
I've forgot speed rate but I let machine take a break every 5 min. of 30 min. running
'cause I run Dry and don't want to..o..o..o messy for the sign. Whole sign dimension is: 72" x 24"
By the way, If anyone know where I can find the Shopbot file to RE-Surlface for particle board table, I appreciate it.
Sorry for my English.
Uncle Hai
6239

[Andy (Unregistered Guest)]

Just cut a load of 0.50 aluminium for channel letters.

I used a 3.95mm Trend spiral cutter ground for up cutting- worked a treat- in fact it cut as easy as soft PVC sign board.

My letters were only 6" or so I kept the feed to around 12- 15" p/m but the results were perfect- I was a bit surprised to be honest. I'm doing some 3ft high ones next week and I'm going to up the feeds to find out the max useable rate.

Trend cutter was around £15 and it's still real sharp. Don't know if they are available in the US as Trend is a UK company- I think?

I was using misting with a light maintenace oil but I don't think this is really needed- the chips were flying out on the test parts which were not misted. (my mister is a basic air tool automatic oiler system which I adapted and cost about £30- works perfectly)

Vacuum is essential as the thin sheet does tend to chatter a bit.

I started out with down cutters but have recently swapped to up cutters and the difference is amazing- no weld backs, no snapping and much quicker cuts and better results. I also have endmills which came with my CNC system but I've found them to be too harsh for signmaking materials and use only spirals. With a 2mm diameter Trend bit I managed to cut some 1/2" high 1/4" thick Plexiglas for a metal casting template- worked out a lot better than I though it would.

If you are making channel letters from ali I've been using an aluminium brazing/ welding system that works off a rod of material that you feed into the joint with a propane gun- works fine and a whole lot cheaper than tig or mig setups.

easyweld.com or .co.uk- can't remember which at the moment.

Hope this helps

[Call-Tech]

I have been meaning to try the O bit everyone mention, but I can't find one locally and did not want to order just one bit online.

I was using a 1/4" down spiral mill. If my math is correct a 3.95mm is closer to a 1/8" cutter. That is the size that WCSC mentioned also. I had not concidered using a smaller cutter. Andy's speed is slower than I tried. I cut in inches per second, but 15" per minute would be .25 inches per second, I believe I was running .5 - 1 inch per second and was melting aluminum. I would prefer to cut dry as I don't want the added step of removing oil from aluminum before painting or applying vinyl.

[WCSC (Unregistered Guest)]

Removing oil is the easy thing. Rag & Laquor thinner