Help with cutting 6061 Aluminum sheet stock?

[Decks]

81.jpg
I recently bought an older PRT Alpha with a 5HP Colombo spindle, Vacuum table, proximity switches, etc. for the purpose of cutting 6061 aluminum sheet stock. I can get 81 pieces out of a 48x48x0.375 sheet. The problem is I'm going thru 3-5 bits per sheet. I'm using a Freud 1/4" solid carbide 2 flute upcut, with compressed air constantly blowing on the bit. I've tried cutting oil, but it doesn't seem to help much, plus it ruins my LDF tabletop. I'm cutting at slow speeds 1.0, 0.4 and only taking off 0.01 per pass. It takes a LONG time. Any suggestions? What am I doing wrong? Attached is a photo of the finished sheet. Sorry, first time using the forum, but long time Shopbotter.
Thank you,
Jeremy

[knight_toolworks]

well your bit first off a 0 flute will last a lot longer. you have to test the pass depth out with each bit if you start to see a burr or bit gumming you need to reduce the pass depth but I have cut upto 1/18" in pass. holding the parts in place is the trick. what rpms are you using? you should be doing a climb cut too. no need for cooling on that stock.

[Burkhardt]

When you write "going through 3-5 bits/sheet" do you mean the bit breaks, does it become dull or do the chips weld onto the bit? Depending on the failure mode the cure may be different. I also use o-flute bits when I have them but I have also successfully cut with special TiAlN coated 3-flute bits made by SGS for aluminum (at only 8-9krpm). They are less fragile than the o-flutes.

If there is a pocket or other bulk removal, I will try to cut a very small starting pocket with shallow depth steps (say 0.01 or 0.02") and remove the bulk of material with a full depth cut and small horizontal step-over. This side cutting strategy uses more of the flute and it lasts longer than having the sharp bottom flute point(s) do the work.

Although it is messy I normally use a 50/50 mix of water and isopropyl alcohol with a drop of liquid soap from a hand sprayer as coolant. Just keeping it slightly wet prevents chip welding. No need to flood it and the mixture dries up rapidly. That said, I have an aluminum table and a spill won't matter.

[MogulTx]

I cut a fair amount of aluminum and used to do it on a PRT. It only had a PC Router- so you should be doing OK with that machine. Hopefully it has good (higher ratio) steppers....

When I cut aluminum, I usually use an Onsrud Spiral O, single flute, like the folks above are indicating. I usually work at 1.7 / .43 for small bits. It is VERY important to RAMP the cut! I usually use .025-.032" per pass. I do not usually use a coolant or venturi air. If I lose a bit, it is usually because I have erred in moving the spindle- or that the bit has warmed up a little and some aluminum got welded to it. Not really common. I also cut using a spindle these days. I am at 4hp, so it would be fairly comparable to what you are using. I can't recall what speed I use for the spindle, but I usually start in about 14500, make certain I have a SHARP bit, and listen carefully to the cut as it starts and progresses. if you hear sounds that are not smooth and uniform, you probably have a problem. Some of the bigger culprits are chatter, heating, table uniformity, etc. When I do parts like yours ( many multiples, with holes through them) I will always clamp my workpiece down in several places and begin my through-hole cuts. As these are completed I go back and put in deck screws to hold the parts firmly down. Then I run my periphery cuts... and the screws prevent the parts from chattering or moving- saving you a lot of headaches.

Look for posts by Brady with reference to aluminum cutting. He was instrumental to me getting started down this track.

This will get you more than started and should bring down your cut times and your frustration. Buy the BEST bits you can find for this. The largest bit that will still do your smallest feature ( so that you have the most rigid bit with a greater cutting edge and more mass and length to dissipate the heat. This will cost a little up front and if you are not careful, will cost you in losses! But it should save you in time, lost bits and quicker cut ability. Once you are successful at a MODEST speed, increase your cut speed and spindle speed until you have reached and then exceeded your best cut quality. (TAKE NOTES) Then back it down until you reach what you think is the best. THAT is your spindle speed, travel rate and plunge rate to use. SAVE OFF THAT TOOLING NUMBER AND THOSE PARAMETERS in your tool set up... Best of luck to you. Monty

[MogulTx]

And I am cutting on a 60 x 60 sheet of .12 material this afternoon. Yesterday was a 60" diameter in .25 thickness. I often cut this using an 1/8" diameter bit. It is really a matter of practice and patience...

I checked and my bit is an Onsrud 63-610 (1/8" for tonight's work)

MGM

[Alex Naumenko]

.25 Single O flute. 24000rpm 120 ipm for XY, 45 for ipm Z. 0.80 pass with cold air gun.