Cutting Aluminum

[phardy79]

I have a client that wants parts cut from 1/8", 1/4" and 1/2" aluminum. I will be using a 1/4" end mill. What is the proper spindle speed and feed rates for this material? I have a compressed air line to cool the bit. What are the other tips and tricks for cutting this material? What are the best kinds of bits? Thanks for any advise on this issue.

[scottbot]

Paul,
I've only cut (5/16") Aluminum once.
I was using a 1/4" double edge upcut spiral (Onsrud 81-204) which was recommended to me by Onsrud.
About halfway through the material the chips started to re-weld to the bit. I was using compressed air with a cold gun to cool the bit. It didn't seem to make much of a difference so I quit using it.
Out of desparation I started squirting WD40 on the bit as it was cutting. It worked like magic and I used 2 cans to get the job done. The cuts were nice and clean with no burrs.

I was cutting 14" high letters out of a 48" square sheet. When each letter cut through the sheet would buckle a bit and I would lose a lot of hold down vacuum. I had to stop the job after cutting each letter to vacuum up the cuttings, clean the area with Windex and tape the cut with packing tape to keep the sheet tight to the table.

The job would have been a nightmare without the WD40. I did my research on this forum before attempting to cut the Aluminum and it seems that others cut Aluminum successfully without any cutting fluid. I guess it can be done but it sure wasn't working for me.

I hope this helps.
Scott

[Brady Watson]

There are many posts here regarding cutting AL. Use the search function.

Generally speaking, AL can be cut dry using a single spiral-O flute bit run at 1 IPS and 13-15000 RPM. Care must be taken to ramp into the AL rather than plunging straight down. No lube/WD40 or air cooling required for most alloys.

-B

[woodworx]

small stepdown, high feed rate, low rpms, lots of hold down. Trial and error=Success!

[blackhawk]

Paul - I have only cut .050" thick aluminum with my Shopbot so far. At my real job, I do run a Bridgeport milling machine once in a while. For a 1/4" endmill, I would probably run the Bridgeport at 1500-2000 RPM with a feedrate of 12-20 inches per minute. Air cooling will not hurt anything here, but I don't think that you get much of a benefit. I have not used any Onsrud cutters, but for the Bridgeport we generally use standard aluminum cutting endmills purchased from MSC. Putnam is a pretty common brand and TiCN coatings really help with wear on the tool. My speeds and feeds are pretty conservative because I am not needing parts for production. I normally only cut 1/16" deep per pass with a 1/4" endmill. I like to start conservative and bump up speeds, feeds, depths of cut if things look good. Sometimes the quality of the aluminum can make a big difference.

[woodworx]

I have cut everything up to 3/4" 6061 for 10+hours a day sometimes. AL machines ok on the bot, but until you experiment yourself, there is no one answer to your question. Ideally cut from a sheet the entire size of your bed, that is if you have a vacuum, to retain full vac pressure. Less movement=less vibration. Less vibration will give you the smoothest cut. There is no sanding tricks after machining aluminum, so you only have one shot to make it correct. Talk to bit mfgr's about their bits, but every machine is different. Like most of my projects, just jumping in neck deep is the only way you get things done. I would by 2 bits, so when you wreck the first one, you have back up.

[harryball]

So... before I myself start working on this 3/8" 6061 aluminum plate to cut a bracket I need let me see if my lurking has properly informed me...

Using a 1/4" O-Flute 65-025 Onsrud bit.
cutting climb
.75 ips
10k RPM
using some air to blow chips clear and cool
ramping all cuts
.07" passes

Am I missing something?

/RB

[phardy79]

All, Thanks for the great info. Robert, thanks for your to the point answer. This will give me a great starting point.

If anyone else has any suggestions, please feel free to comment. I would love to here your successes and failures.

[Brady Watson]

Paul,
Buy an extra bit of material & TRY IT! We'd love to hear about YOUR success!

It wasn't long ago when AL was considered nearly too exotic to cut on a SB...many of us who cut it didn't have the luxury of comparing notes with anyone else.

I'll be cutting carbon fiber sheets today on my Bot...There's not much I haven't cut (or tried to cut) on my machine.

-B

[harryball]

I finished my bracket, photos attached. It's about 20" at the longest and the holes are 3/8"

Designed and toolpathed in Aspire.
I cut at .8 ips and .5 ips plunge rate
10k RPM
.07" passes
Ramped all cuts for 1"
Cut in the climb direction and visually confirmed the best edge is the climb side of the cut.
The holes were cut with the same 1/4" O-Flute bit, I used a spiral tool path setting in the ramping.
I manually held the air hose to it to keep the chips clear and for cooling.
I started with a vac holddown only through my regular bleeder board and cut the holes. Then I added screws to the holes for improved holddown and cut the outside large by .02" I then followed that with a final single full depth pass to clean up the .02" oversize.

The cut went without excitement.
The results were good but you can see the tooling marks. Before the clean up pass it was obvious that it was cut in multiple passes but still not a bad finish. The single final pass really cleaned it well. I cut at the same speed for the final pass, perhaps speeding up / slowing down either/or the cut speed and RPMs may have improved the final quality as maybe a different bit might. But I'm very happy with the results here.



37481.jpg

37482.jpg

/RB