..... Aluminum Again

[john_l]

Sorry.

I know about all the other aluminum threads here but thought I would ask anyway.

It has been a while since I succesfully cut .125 aluminum on the bot. I cannot find the settings I dialed in before and right now have an urgent need to get a couple parts off the machine.

The attached picture shows the trainwreck I have now. My machine is a PRT, 3hp spindle. I am using a 63-725 Onsrud bit, at 12000 rpm, X/Y at 1 ips, Z at .4 ips. I do not know what type of aluminum this is... it is .125 sheet that came from Harbor Sales.

I tried speeding up and slowing the spindle, and also the X and Y. I just couldnt improve the cut so I aborted it before doing damage to my machine or sending a broken bit out of bounds.

Would you say this looks like dull bit? too fast/too slow rpm? too fast/too slow feed? I am really at a loss. Thanks.


6472

[steve4460]

try 10000 rpm at 0.5 feed and 0.5 for the Z and a squirt of WD40 with a downspiral bit single flute.

[coach]

I am cutting .080 alum tomorrow. Last time I recall feed of 0.8 and around 12,000+
I don't recall the bit even though I just put it in the spindle today for the morning.

[coach]

as Stephan stated. I also sprayed the sheet with wD40 prior to cutting.

[bernott]

John,

Look like low grade al to me!
12 to 16000rpm and .6 or .7 x/y and ramp in.
also some type of coolant is a must.

[eaglesplsh]

I hate it when that happens!

I have a couple aluminum jobs coming up this week, so I'll be contending with the same issue... We just upgraded to a PRS Alpha, so I've got to dial in all new feed/speed rates as I redo all our cut files.

My old rates from our previous machine probably won't help you. But, I can say that you're using the right type of bit. While WD40 may help you, I never found it necessary once I got my feed/speed rates right.

It looks like your chips are welding back to your piece, which would mean one of two things:

your feed rate is too slow/RPMs are too high - reducing your chipload so the chips aren't removing heat from the bit fast enough

or

your bit is dull and getting hot from friction/rubbing on the metal instead of slicing through it

Judging by your picture, I think that you will be able to cut this alloy once you dial in the feed/speed. Many aluminum alloys are designed to be stretched into 3D shapes. If you tried to cut one of them with you're router, it would look like you'd been stiring molten peanut butter (you wouldn't see the chips that are in your picture.) These metals are soft and gummy - perfect for stretching without tears, horrible for shearing with a sharp blade. I once had a couple tons of this "forming" aluminum to cut and a factory full of CNC mills to cut it with - we ended up sending the job out to be cut by water jet.

Best of luck!

[carlcnc]

I cut a lot of aluminum,mostly 5052[soft and "gummy"] also 6061. everything from .04 to 1"
to me the key has always been depth per pass
vs dia of cutter,I use single flute up spirals from RL Schmitt, usually 3/16-1/4.
to avoid heating , max depth per pass is .04,rpm 15-18000,. feedrates from 30ipm [.5 sec] to 90ipm[1.5 sec].
I don't like using WD40 as it takes MEK to clean it before any painting. switched to a few drops of bar-n-chain oil IN the cut every other pass.
Brady will attest that even a small amt of air
is also very helpful.
Its amazing how long a cutter lasts in aluminum IF you can keep it cooled,
Carl

[coach]

I cut some alum today. Was .065 not 080 as I thought. I used an Onsrud 63-620 1/4" bit. Feed was .8 IPS and Z was .5 the speed was 12,600. I did in 2 passes but cut the sheet in half in 1 pass and it was as clean as 2 passes. Parts needed no clean up except blowing chips off. I also spayed the sheet with WD 40.
6473

[john_l]

Thanks for all the suggestions. I ended up switching bits to an Osrud 65-025 and slowed my feed to around .8 and got much better results. I also tried the WD40 sprayed on the sheet and it didnt make any where near the mess I expected, and seemed to help a lot.

I had thought that 63-725 bit was the one I had used previously but I must have been mistaken as Onsrud lists that as a plastic cutting bit. So maybe thats another reason why I was getting such horrible results also.

I just ordered an Onsrud 63-620 to try next time and i am also going to look into bits from Schmitt.

Thanks to all!

[ron_moorehead]

Look at getting some end mills designed for cutting metal and aluminum, I found some very nice end mills for about $10.00 each and got some new collects for my spindle to fit the end mills in 1/8" 5/16" and 3/8".