Cutting .050 aluminum

[vitals]

I am a new user and and having a hard time with cutting .050 prepainted aluminum for channel letter backs. I am using a Onsrud 63-606 up bit and have tried many many settings.I have a standard shopbot with a Porter router.I can get an OK cut, with a slight buhr on the top edge and my cuts have slight choppyness on the edges. I am screwing the 4' x8' sheet down to the table with cardboard between the sheet & the mdf top. Can anyone give me advice on feeds & sppedsfor this typeof setup?

[erik_f]

I have no idea on something that thin...but my first gut feeling is to use a straight bit.

[woodworx]

straight bit 1/8". Air spraying on the cut. LOTS OF VACUUM power.

[vitals]

I do not have a vacuum table

[road_king]

John,

I have never cut aluminum on my bot yet.

I have used a down spiral bit on 3/4 " maple plywood and get nice clean "top edges". My first time using an up-spiral on the same 3/4" maple plywood, the top edges were "fuzzy".

Maybe a down spiral or a straight bit would be better!
GB

[Brady Watson]

You need to use vacuum to hold down the AL correctly, otherwise forget it. I'd tell you that you can use carpet tape, but you'll bend the AL trying to get it off of the machine.

A single spiral-O flute is the weapon of choice.

-B

[hol]

Single up cut spiral - works great. We cut alot of aluminum that size without a vacuum hold down.

.040,.050, .080. no problem once you get everything dialed in.

We just take the sheet and screw it directly to the spoilboard wih nothing in between. Using the porter cable router at full rpm's (21,000) typical speed for small letters is pretty slow, usually .65 ips with an 1/8 inch bit just to keep the bit from breaking in any tight corners of the cut. Larger shapes and letters we cut at 2 ips with a .25" single flute upcut spiral.

You can see some examples on our site in the CNC routed section to see how clean the bot cuts the aluminum.

[vitals]

thanks Larry, do you coolant? Any other tips?

[hol]

No coolant- usually cut conventional instead of climbmill.

The main thing is to find a way to keep the aluminum sheet from rising up on the bit - without using your hands- of course! A good way is to screw the sheet to the table on the sides - then drill pilot holes in the sheet where there is no artwork to be cut. Then you can use those holes to screw the sheet to the table on the interior of your aluminum which really helps told it down as the router cuts out your shapes.

[magic]

Larry is right on.

[robtown]

Different alloys will have different cutting characteristics. I have a PRT upgraded with a 4g board. I don't do aluminum often, but when I do I would say I shave, not cut, my way through it with thin passes and coolant or compressed air.

[blackhawk]

I just tried cutting .050" painted aluminum for a friend of mine. He got the pre-painted aluminum from a trailer mfg company. These are the trailers for road tractors (18 wheelers). My friend runs a machine shop, so he gave me a 2 flute HSS metal cutting endmill which is an up spiral. I ran my Porter Cable at 10,000 RPM and 10 IPM, only taking .010" passes. It seemed to cut like butter with hardly any burrs. I know that is slow with a light cut, but it worked. I sprayed some compressed air on there intermittently, but I don't really think that I needed it.

[Brady Watson]

I've cut many different types of AL alloys on my machine from .030 to 1" thick stock. While there are probably some of you out there cutting metal sheets with a screw popped in 'here or there', don't be fooled about the importance of holding the material down to the spoilboard effectively. Screws can bow & warp the metal and cause the sheet to lift up and ride the bit. If you want to do it right, hook yourself up with a vacuum hold down system. (search for the open source vac thread that I started, esp. you are on a budget) If you are only doing it from time to time, then a screw here and there or clamps & carefully thought out tabs will likely do. Keep your eye on the surrounding area as you tighten down the screws...don't go too tight.

Coolant is most likely not needed for .050 - but if the alloy commands it, then there are several threads on here discussing how to make your own cooling setup - as well as the proper RPM and move speed to get you in the range. Cranking the RPM all the way up isn't the right speed for everyone, and the diameter of the bit also influences RPM & cutting speed as well as the need for coolant. A good general setting for AL sheet is 1,.4 IPS and 13k RPM with a 1/4" single spiral-O. If you are using PartWorks be sure to ramp into the cuts. Straight plunges are a no-no in AL.

While you might be able to get away with just 'winging' it with thinner material, things get more critical as the AL gets thicker. Thinner AL sheet is much more forgiving of incorrect feed rates, speeds and RPM than thicker material...Keep that in mind for those reading that want to cut thicker stuff. Hold that metal down or somebody could get hurt. AND as I have said before - SAFETY GLASSES ARE A MUST!!! Static electricity WILL shoot AL towards your eyes when you lift the sheet off of the table...a word to the wise.

-B

[paco]

I use the 62-600 series (spiral down 1 O-flute) to cut thin AL (less than 0.065") in a single pass for cutter of 3/16" CED or more. This help the vacuum action and keep the material down on the spoilboard. Up cut will lift the material and make it vibrate, eventually ruin the parts or snap the tool.

16000 at 0.5 to 1"/sec., half that for the Z for a single fluted tool, less RPM for a conventional spiral up 2 flutes AL end mill. Like Brady said gentle ramping in is a must. Just air to keep that tool cool.

I haven't been able to get consistent (good) result with soft (3003) utility AL. Will almost always burr/melted. I wish I could find the fin d the trick with it if there's any... I "always" buy the AL I cut and I buy only 6061T6.

[rb99]

"I haven't been able to get consistent (good) result with soft (3003) utility AL. Will almost always burr/melted. I wish I could find the fin d the trick with it if there's any... I "always" buy the AL I cut and I buy only 6061T6."

Have you tried Alumacut or similar coolant/cutting fluid?

Also if it is melting it is too hot. This might be too slow on the feed and too fast on the router.

A dull bit will give problems, and without fluid you will dull them fast. You could try hand misting with spray bottle.

When it first starts melting, stop and check the bit for small deposits of aluminum.

With a new bit does it cut ok for the first few feet or inches?


RB

[paco]

My "best" result in utility AL was with a 1/4" CED plastic straight edge (1) O-flute in a single pass at fast rate. The cut was fine then for a length of say 6 to 12" it was just smearing until I stop it to remove the slag in the tool flute. I tried various lubricant but I haven't seen any improvement on my end and I had to clean the part before delivering it to the customer.

Do you cut 3003/utility AL on a regular basis with success?

[hol]

Brady brought up a good point about straight plunge - definately ramp into the aluminum even on the thin stuff. Straight plunges not only will help you break bits but will shoot a very hot piece of aluminum off the table from when the bit first pierces the aluminum -and the last thing you want is to be hit in the face (or eye) with that.

Last year we had to drill 16,000 .25 inch holes into 1/16" aluminum square tubes for a table top display project - with no way to ramp into the cut. Even with the guard around the bit we had shards of aluminum everywhere.

[Brady Watson]

Larry,
Next time you need to do some drilling, try an 'EasyTorque' drill bit. Drills thru AL like butter as fast as you want to go with pretty curly shavings. My supplier calls them Easy Torque...if you want more info I'll have to call him to get it for you.

-B

[hol]

Thanks Brady - I'll keep that in mind!

[scottbot]

Hi John,
A little while back I cut 13 letters from 3/16" Aluminum. I used a bit (don't remember right now and don't have the info handy) recommended to me by Onsrud. I researched feed rates and RPM etc. on this forum before I started anything. I have a vacuum hold down.

I was taking light cuts. Probably around 0.030". I also had a cold gun blowing really cold air on the bit. I wasn't using any lubrication.
The first letter started out great and I was encouraged that the job was going to go well. About halfway through the material the Aluminum started to reweld to the bit. Most likely I was using the wrong bit, feed rate, RPM or all of the above. I didn't really have the luxury (extra material) to play around with the settings so I simply got a can of WD40 and started to spray the bit. It worked like magic. Although it was a little messy the rest of the cuts were nice and smooth with no burrs or chatter marks.

I echo the other comments about hold down. My material would buckle and lift off the table after each letter was cut so I had to shut it down, vacuum the cuttings, clean it with Windex and tape over the cuts to get enough vacuum to hold the sheet down. Do the best you can with your hold down because you are going to need it.

Good luck.

Scott

[woodworx]

If you have a chunk of AL that is stuck to the bit, throw a bit of machining wax on your bit and keep cutting. The piece should come off. Every once in a while put a chunk of wax in the path of the bit. You will find it helps. Vacuum power has always been the 1 true help in machining aluminum. Less vibration, and movement through out the cut will keep the cuts consistent and keep the piece from riding up on the bit. Never use a down spiral on AL.

[Brady Watson]

"Never use a down spiral on AL."

Amen to that!

-B