Cutting Speeds?

[joewino]

I'm sure this has been asked many times before, but I'll ask again:

Is there a chart or listing anywhere that has recommended spindle speeds and feed rates for various materials?

I am especially interested in aluminum - 1/8" to 1/4" thick...and I know that there are various types of aluminum, but this would be for sign faces for use with push through acrylic copy.

Any suggestions would be greatly appreciated. This forum is tremendous. It has already helped me considerably.

[wcsg]

For push thru acrylic copy why so thick? What sign type is it? I've done some cabinet's 4'x 18' and used .080 all around with 3/4" push thru copy. Using 1/8" to 1/4" your not going to get much copy passsing thru as you also have to decide on a flanged rear or using a solvent to adhere

[joewino]

Sorry...didn't make myself very clear. I will be doing some profile cutting in thicker aluminum (possibly up to .25") and also some push through type faces using something closer to.080.

There is not a job to do right at the moment, but I'm just planning on some samples and need to know what are the correct speeds.

[wcsg]

I use polished spiral bits from Belin tools

I use both a 1/8" Ced & 1/4" all z speeds @ .30IPS

on 1/8" CED I'm going 18k RPM @ .40" IPS
on 1/4" CED 12k RPM @ 1" IPS

Acrylic

on 1/8" CED I'm going 18k RPM @ 1.25" IPS
on 1/4" CED 15k RPM @ 2.5" IPS

6061 is harder alum while 5052 is softer, the softer get s a little hotter and is much cheaper I usually use 5052 and shoot a little wd-40 every 30 secs or so

p.s. enjoyed your seminars at long beach on design

[joewino]

Thanks for the info, Erik. And the nice words about the seminar.

One more question: do you do each in one pass or step down with the thicker material?

[wcsg]

You can go the depth the same as the diameter of the tool. 1/4" CED 1/4" depth pass. Tooling manufacturer's shutter at 5052 and recommend 6061.

[scottcox]

Raymond,

I'm finding that my sweet spot with 6061 aluminum is 1/16" stepdown and 1/16" stepover, climb milling at 1 IPS at 15K rpm (5hp spindle). I'm using WD-40 for lube and no compressed air or mister. The bit is room temperature after cutting and the edge is very clean.

I tried to do a matrix of all the different speeds and feeds (for aluminum) mentioned on the forum and found that they were all over the scale. After talking with Onsrud, I got a good starting point and experimented from there.

BTW: Onsrud says 2IPS @ 18K and 1/8" stepdown. This worked but the cut was ugly and it heated my bit up until it finally broke. Now THAT was fun. Not.

Good luck and please post your successful feeds and speeds with aluminum.

Edited to include.... I was using a 1/4" CED bit.

[wcsg]

Forgot to post my bits

33317 1/8"CED 5/16" CEL 1/4" Shank
33635 1/4" CED 5/8 CEL 1/4" Shank

These are single flute spiral O bits made for alum, brass, and copper. I can't tell you how great the harmonics are while cutting. Good Luck and be sure to tell us how it went