What is "good performance" for cutting aluminium?

[mitchejc]

This might be a bit if a daft question but I'm vaguely starting to see the light at the end of the tunnel in my build and I'm just trying to manage my expectations here. What would be considered "good" performance for profile cutting/slotting alu on a DIY 2.2kw gantry type router in terms of dept of cut and feed rates with a decent surface finish? I'm taking about real world numbers for routers here and not the stuff that is spit out by the feed/speed calculators for high speed/ high power VMC's. I've been cutting alu for a long time on my big router and my best surface finish for slotting/profiling is at around 1000mm/min, 0.5mm depth of cut and 14000rpm with a 6mm cutter. I'm hoping for better with the new machine. What's your experience with your machines or any thought on what "good" performance should be?

[Boyan Silyavski]

I would say same as before but without the scratching :hysterical: . Say 3-6mm pass depth and a bit faster.

You new baby will do even better but i find that pushing something too hard results in short life of something else.

[mitchejc]

haha, scratching, good one silyavski. So, you're say at 0.5 mm DOC I can save cutters as I don't even have to start the spindle, the machine with just scratch it through :-) Ok maybe I'm too gentle on my tools.
3-6mm is huge. I'd be EXTREMELY happy with anything remotely like that. Is that what you could do on the yellow steel machine?

[Boyan Silyavski]

haha, scratching, good one silyavski. So, you're say at 0.5 mm DOC I can save cutters as I don't even have to start the spindle, the machine with just scratch it through :-) Ok maybe I'm too gentle on my tools.
3-6mm is huge. I'd be EXTREMELY happy with anything remotely like that. Is that what you could do on the yellow steel machine?

3mm depth of cut will be fore sure if you don't make a major mistake.


The yellow machine i have never had the possibility to push it to the limit. remember there is only 0.8kw spindle. But yes, i have tried it with 6mm bit at up to 1.5 mm depth 650mm/min as i remember and it cuts it like butter. Now the other thing is not the speed but the finish. Its perfect. Thats more important to me.

[mitchejc]

That's very good news. You are so right, whatever the speed, the surface finish has to be perfect.

[Web Goblin]

Although the above posts deal with router cutting or milling the cut quality on the part is quite good. You can improve the corners by quite a bit by having external loops or corner routines on them.

[Blackrat]

i think the diagram is the wrong way round ?

[axmem]

U said u are to gentle for your tools? U are actually ruing your tool edges going with small depths as the rest of the tool does nothing. Think about going 3mm deep at f800 and u are using more of your cutter cutting surface and won't forcing machine as u going slower but cutting more... So just the thought

[mitchejc]

Thx, yep you are correct about killing the cutters quickly with those shallow cuts, I meant to say I'm too gentle on my old machine. Will do a test cut at 3mm doc cut @ 800 and see how it goes. +- what RPM's are you running for that?

[axmem]

Biggest trouble with cutting deeper is the swarf removal ratio. How do you cooling your tool?

[axmem]

I cut aluminum on Haas at work. It's a big machine and very powerful so I can go as fast as I want. But big trouble with aluminum is faster your spindle spins more heat produces that causes tool to stick to swarf.

[mitchejc]

I've got a compressed air nozzle mounted on my Z that is pointed directly at the cutter to blow the chips away but I do not have an auto misting/oiling unit. I manually just give it a short spray of Q-20 penetrating oil every 30 seconds or so. The Q20 seems to work ok as I did not have any alu welding to the cutter in a very long time.

[axmem]

U said u need a good surface Finnish will it be better do roughing cut first to let the tool work hard and than just go over and Finnish the job?

[axmem]

There are no good or bad formula for speed and fees what counts is time of cut and wear of cutter. Generally depths of cut is the radius of cutter (to be safe) if your machine can handle it. But deeper u go deflection starts to kik in

[axmem]

So taking that to account make sure your tool sticks out of the collet just enough to reach and be safe with clamps etc.

[JAZZCNC]

I find using a 3 flute carbide roughing cutter then full depth 0.35mm finish pass with twin flute is best setup with aluminium using 2.2Kw spindle.

I can easily cut 5-6mm DOC slots with 8mm serrated edge roughing cutter between 900-1200mm/min 15000-20000rpm. This setup gives me good material removal rates along with excellent finish and best tool life.
Using above rougher I can cut 10mm DOC when pocketing with 45-50% step over.

In all cases using air/mist.

[mitchejc]

Thanks for the info. I have not tried the serrated roughing cutters yet so I'll try and get some to give a go. It some stage I have tried a finishing cut of 0.1mm but I did step down and it did not really make a big difference to surface finish. I'll try 0.35 and full depth.

A few weeks ago I was spot drilling and cutting 25mm thick alu parts for my new machine, it was late and I was tired and I managed to not zero Z after switching tools from a short center drill to a brand new 6mm 2 flute carbide cutter. Hit start, machine went to part 0,0 and from there it ramped into the material on the way to the pocket it was supposed to cut. Sounded like the rumble of the apocalypse and I somehow managed to hit estop before the cutter snapped. I measured it and the accidental slot it cut was +-4cm long and 8mm at it deepest spot. Not a great experience but it has given me a bit of confidence to try slightly more aggressive cutting parameters on my old machine.