Speeds and Feeds for Alum

[WB]

I have a couple signs that need to be cut/engraved in 3/16" Alum. I'm using a 1/8" carbide bit with 2 flutes. I'm only going down about .06" but I'm having a hard time getting a nice finish. It could have something to do with the $13 bit but I thought I'd as about what speeds and feeds everyoen runs.. I've tried 15000RPM and 30 IPM and 22500 and 25IPM and I'm still not happy.. Any advice?

I know the quailty of bit matters, I do have some Onsurd single flute bits buit I called my suppliers and wanted something really small, (3/64") so I thougth I'd try these out.

 

[Westcoast Sign Guy]

Those feeds and speeds area a good starting point, what is your hold down method, is it solid? ANy vibration and your finish is crap.

Personally I only use Belin, $33 a bit single flute but nice finish.


Is this a 1/8" spiral flute your using? 1/8" CED? Or a engraver bit?

 

[Signguy9311]

Are you keeping the bit cool? Spraying soapy water while it's cutting helps keeping bit cool. Single straight flute bits with DOALL grease works the best.

 

[CES020]

A recent tech support call to Onsrud about this same topic told me to run it in the 8000 RPM range with .003-.005 per flute chip load. He said one of the most common mistakes with router owners cutting aluminum is they run way too many rpm's.

I tried his suggestions and found his recommendation to be very good. I had been taking multiple light passes, now I'm able to do one pass, so it's a slower feed, but it's finishing the job quicker.

 

[CNCCookbook]

There is a surprising amount of complexity associated with feeds and speeds, especially for metal which can have a pretty narrow "sweet spot".

In terms of your 1/8" cut, 0.06" deep, if I run those values through our G-Wizard feeds and speeds calculator, I get a recommendation of 40 IPM for 20K rpm, 30 IPM for 15K rpm, and so on.

The chipload and rpm are going to vary based on the size of cutter, which is important too.

However, and this is key, how far out does the cutter extend from the collet? An 1/8" is not very rigid. You could be getting tool deflection that spoils your finish. If it sticks out 1" (that would be a LOT for this size cutter), G-Wizard predicts 0.0014" of deflection, which is way high.

At 0.5" of stickout, that deflection drops to 0.0002", which is about what you want for decent surface finish on a cutter this size. So, I certainly would make sure it extends no more than 1/2" and preferably even a little less.

Another thing about aluminum is it wants to stick to the cutter. WD40 works pretty well to minimize that. Shoot a little WD40 from the can onto it every so often as it cuts and see if that helps.

Best,

Bob Warfield

 

[WB]

Thanks for the input guys.. We actually ditched the project for a couple reasons, 1. it was cutting like crap and 2. 1 of the signs was very very very very small. I had order some 3/64" bits and when I ran my simulations they were still to big to give me the detail I wanted.

That being said I'd still like to get this alum. cutting down.

 

[WB]

A recent tech support call to Onsrud about this same topic told me to run it in the 8000 RPM range with .003-.005 per flute chip load. He said one of the most common mistakes with router owners cutting aluminum is they run way too many rpm's.

I tried his suggestions and found his recommendation to be very good. I had been taking multiple light passes, now I'm able to do one pass, so it's a slower feed, but it's finishing the job quicker.

what exactly does the chip load mean.. is that in/min per flute? that can't be right!?

 

[artbot]

what alloy? 3003? 5052? if it's 3003 you are going to have difficulty compared to other alloys.

and go single flute with any fluid you can get you hands on, even soapy water in a squirt bottle works fine.

 

[CES020]

You take the chip load, multiply it by the number of flutes and then multiply that by the RPM. That'll give you the inches per minute. If you want inches per second, just calculate that from there.

So if it's 8000 RPM with a .004" chip load, using a single flute cutter, that would be 8000 x .004" x 1 = IPM.

So, that would be 32 inches per minute or .53 inches per second.

If you had a 2 flute cutter, it would be 64 inches per minute or 1.06 inches per second.