Tips for cutting 1050 aluminium

[d4cnc]

I have two air nozzles at around 90 degrees blowing towards the vacuum cleaner nozzle.. so I was hoping that would be ok no matter which direction the cutter was moving.. I guess it would vary in effectiveness depending on what direction it cuts..


I've got some Draper cutting fluid here that I can use.. or is WD40 more recommended? I can pick some up this evening.. Off to get some carpet tape now. Is that the recommended tape? Ideally I'd like to put it straight on the MDF spoil board if possible? Or shall I get some spray adhesive?


@sinnsvak - are you using single flute? Which aluminium grade are you using?

[sinnsvak]

Single flute all the way with 6040 machines. Tried others, but my machine cant handle it. I think the grade Im cutting the most in is 6082, but I also have some unknown 5mm plate which is very sticky, but the speeds also work well on that.

Each machine, especially our type, varies so much in quality that we probably get different optimal speeds and feeds. I know the settings I posted is right for my machine because:
#1 the finish is great
#2 the sound when it cuts is like music to my ears
#3 the cutters last forever. (been on the same cutter since november, and cutting aluminium 10-20h a week.

WD40 is good stuff, but it is more messy than alcohol, which I get for free from work.


Cutting is one part of this, but fixturing sometimes takes the longest time to figure out. Try different methods and go with what works for you. I often use screws into the spoilboard to keep things in place and flat.

[d4cnc]

Ah I see, yes they appear quite different some of them looking on eBay now..


Thanks for the advice.. I ended up picking up some carpet tape.. normal double sided.. carpet spray adhesive and removable bluetak spray adhesive (never heard of it before)


And the new cutters from Cutwel arrive tomorrow, so I can try again with better work holding.

[Davek0974]

WD40 is the easiest, I am running a paraffin/oil mix which is basically WD but you need to watch the job closely, if the cutter dries out fully it will load up and snap in an instant, there is very little warning.

Here's one i buggered earlier ;)



The copper pipe in front of the cutter is my fogless air/coolant jet, it stopped working and that was the end of the cutter, surprisingly the cutter did not break this time - the machine had enough strength in it to carry on mashing through the metal even though the tool was completely loaded. I never managed to get the metal off the tool as its welded on.

[Robin Hewitt]

I typed aluminium 1050 in to Google and got...
Cold forming Good
Machineability Poor
This is not good stuff for a beginner, suggest you chalk it up to experience.
I avoid the softer aluminium alloys like I avoid cheap Allen keys, waste of money

[Davek0974]

That is a good point Robin, 1050 is 99% pure aluminium, nasty soft stuff but good for deep drawing etc. I tried plasma cutting once - not good ;(

I would go 5251, 5083 or the 6000 range.

[d4cnc]

Thanks for the continued advice everyone. I really appreciate it. What a great community it is here.

I did try and source some better aluminium for cutting, but I wasn't able to find any.. everyone I asked said that they only stocked 1050a at the thickness I wanted. Any tips on where to find some 6061 T6 would be greatly appreciated!


I tried metal supermarkets, themetalstore.. and some others who I forget now..


The one thing is for the 1.5mm stuff, I need to be able to bend it so I believe the 5000 series wouldn't be suitable.. however the 6000 series should be I believe..


It was when I stumbled on a thread here of someone cutting 1050 well, that I thought I'd give it a go using his settings. However, I agree that perhaps it isn't best for a first timer like myself.


The new AluPower cutters arrived, however I'm a little confused on which settings to try next.. I have five 3mm single flute carbides and five 6mm single flute carbides. At £8 each, I'm a little hesistant.
As was previously said a couple of times, every machine is different so I guess there's no 1 magic answer, and some experimentation is in order. However, if you were me, what would be your first setting that you would try next..


I'm considering the following:
Convential milling.. 3mm cutter.. 1.4DOC (0.1mm onion skin?) 12k RPM 400mm/min.. lots of cutting lubricant.. carpet tape.. lots of screws..

[Davek0974]

1.4mm DOC, slotting, 3mm tool, 23,000rpm, 370mm/min
1.4mm DOC, slotting, 6mm tool, 12,000rpm, 550mm/min

Having just been through this, I would pile in with these figures i think and keep my fingers crossed :)

Definitely use lube, WD40 etc, all the way, keep the chips clear.

[d4cnc]

I think I love you guys.


Wow what a difference. The cut was perfect!


I messed up and set the cutter a little too low and so there was no onion skin so the part jumped out and nicked a little in the middle of the long edge. And I need to come up with a solution for not destroying the MDF board with lubrication.. but apart from that.. there was no welding sides.. just lovely chips.


I did 23k RPM & 370mm/min with full 1.4mm DOC.


PS. I just left the old metal on there as a practice with some more screws rather than taping up a new sheet, as I wanted a little practice before ruining another sheet of metal!

[Davek0974]

Nice, thats useful to me too as it means i'm getting a grip on speeds & feeds :)

As you have holes in the part, why not add a g-code pause then bung in a couple of screws to keep the part down??

The mess is a tricky one, my machine is all aluminium so it just wipes off, you could try putting a sheet of paper down first then fixing the plate on that, might keep a fair bit off the MDF bed?