Aluminum feed rate for CNC

Printable View

10-11-2005, 05:34 PM
jayhawksgn

Aluminum feed rate for CNC

Just wanting to confirm some feed rates for cutting aluminum, because what I read is completely different from what the guy who trained me on my ArtCAM software told me.

I have been ordering Onsrud bits from Hartlauer in Orgeon. On his "catalog" it says to cut aluminum with the 63-600 bit at 125ipm with a 1/4" bit. I was instructed to do it at a much more conservative 20-25ipm. Just wanting to get other opinions on how fast to cut, because 1, its time saved, and 2, its important to keep your chipload up, and at the 20-25ipm, chipload is not existent.

And I am cutting .190" 3003 aluminum

Thanks.
10-11-2005, 06:14 PM
Chris D

Need the rest of the story

What RPM and what coolant are you using? Is it a high presure coolant system or a basic flood system?

Chris
10-11-2005, 06:44 PM
jayhawksgn

Its a Kool Mist brand sprayer, and Kool Mist Solution #77, thats all for sure that I know about it.

As for rpm, in the past I have cut this sheet aluminum at either 18,000 or 21,000 rpm.
10-11-2005, 07:09 PM
Chris D

Well, mist coolant is hardly "Great" for high speed machining, high presure flood coolant is much better - so, you don't have an "Ideal" cutting situation.

Now let's look at the math

IPM = RPM X Inches Per Flute X Number of Flutes

So, you have a 1/4" tool bit, assuming 2 flutes @ .19" deep and we will use 20,000 RPM.

.002" per tooth chip load --> 20,000 x .002 x 2 = 80 IPM

That is a moderate to heavy cut based on depth and tool diameter, no flood coolant to wash away chips is another "kick in the butt".

Chris
10-11-2005, 07:17 PM
jayhawksgn

Thanks for the input Chris. I think that I'll find a middle ground between the 20ipm and 125ipm settings. What kind of coolant system would you recommend for this kind of work??
10-11-2005, 07:23 PM
ger21

Download the catalog from Onsrud. They have all the info you need in the back of the catalog. http://www.onsrud.com
10-11-2005, 08:18 PM
Kool Parts

jayhawksgn,
Looks like your only obstacle with that material and rpm is coolant. More is better, just when you think you have enough from all possible directions, just a little more will be just right. Now I assume a enclosed machine. :D
Gary
10-11-2005, 09:00 PM
Chris D

Quote:

Originally Posted by jayhawksgn

Thanks for the input Chris. I think that I'll find a middle ground between the 20ipm and 125ipm settings. What kind of coolant system would you recommend for this kind of work??

As another fellow pointed out - an enclosed machine is best for high speed machining of aluminum. In my experience, high presure coolant is key to flushing the chips out of the cut path and to prevent chip welding and loading of the flutes. The bad part is, I can't recall what PSI is considered high presure for coolant systems (I hate getting old) but I think it is around 100 PSI. There are also cutters specifically designed for cutting aluminum and also coolants that work good for aluminums - talk to your industrail supplier for brands in your locale.
Chris
10-11-2005, 09:22 PM
One of Many

Quote:

Originally Posted by jayhawksgn

Thanks for the input Chris. I think that I'll find a middle ground between the 20ipm and 125ipm settings. What kind of coolant system would you recommend for this kind of work??

This sounds like it is done on a router? Flood coolant would be a bad choice in that case.

Chris gives good information, although the 63-600 is a single flute cutter putting a .002 chip load more in the 40"/min range at 20,000rpm. The mist system may blow the chips out of the path, but I would doubt you can bury the bit in the material at full depth, full width cut and maintain a decent finish. Cutter length will be a factor in that too.

I have always questioned using a single tooth cutter on aluminum. If'n I had my druthers, I'd druther use a 2 flute.

DC
10-11-2005, 11:57 PM
jayhawksgn

Got the job cut, and all went well. Ran the router at 50ipm, 19,000rpm with a Onsrud 63-620 bit.

I did the job in three passes, again mainly to be safe, and the mister was able to keep the path fairly clean of the chips. I didn't have any problems with the chips rewelding themselves except for once when the mister got bumped away from the bit.

In the future I'll make sure that I keep the pressure on the mister as high as I can, and possibly see about getting a second mister if we continue to do much aluminum cutting.
10-21-2005, 06:48 PM
Unabiker

I cut a lot of aluminum with that same bit.
I get the best finish between 80-90ipm, 18000 rpm.
I set the mister to blow just hard enough to turn the drops barely into a mist.
I also get the same chip rewelding if the mist nozzle gets knocked away from the bit.
I was using a 2 flute carbide endmill for this same job before, and the difference in speed, finish, and tool life with the single flute bit is amazing.
11-05-2018, 01:42 AM
cispolaris

Re: Aluminum feed rate for CNC

Quote:

Originally Posted by Unabiker

I cut a lot of aluminum with that same bit.
I get the best finish between 80-90ipm, 18000 rpm.
I set the mister to blow just hard enough to turn the drops barely into a mist.
I also get the same chip rewelding if the mist nozzle gets knocked away from the bit.
I was using a 2 flute carbide endmill for this same job before, and the difference in speed, finish, and tool life with the single flute bit is amazing.

Cutting depth?