Tips for cutting 1050 aluminium

[d4cnc]

Hi,
I did my first cuts in aluminium with the 6040 today, but they didn't go great.
The holes went ok.. (pocketing with single flute 3mm carbide (Alu power from Cutwel).
But when it came the outside contours.. (slotting) I used the same settings and broke the bit.


I believe it may be due to not clamping the 1.5mm thin sheet well enough, and as it was cutting, it made sort of a bend point, and then closed up into the bit trapping it..


However, the finish is very bad too.. Is this type of finish something that is recognizable problem.. too slow feed? Too high rpm? Too deep a cut?


There's not a lot of info that I could find on cutting 1050 (it's not in my HSM calculator) so I went by this thread where someone is suggesting settings that worked.


I used 13k RPM. 600mm/min. 0.5mm DOC. 200mm/min ramp plunge.


The bit broke halfway along a slot on the second pass.


Any help greatly appreciated!

[Davek0974]

Have you got coolant/air/lubricant in there ??

You will get nowhere without it at all on ally.

I am trying to use these exact tools as well but in 2mm and 5mm sizes.

So far i have busted 5 of them including a 5mm!

Have a read through my thread just below ;)

[magicniner]

You stuck the thin material down with carpet tape, right?
Otherwise as you break through your cutout scrap can move around and scrap you, the part or your tooling.
I us a 16mm ally plate to stick down to then clamp the plate to the bed, works great for cut-outs on thin stuff,

- Nick

[Davek0974]

Or, cut/drill all the holes, program a pause in CAM, add some screws through a couple of the holes into the spoil board and then cut the outside.

[JAZZCNC]

1050 is B@#~rd because it's like Cheese string to cut. What your seeing is rubbing not cutting because Chip load is too low and not enough tool engagment so creating Excess heat and melting chips gumming cutter then meltdown of material. I find 1050 is best cut with more DOC so Big chip.

Try cutting with same parameters but at full 1.5mm depth and use Conventional milling. This will produce a large chip and take the heat with it. Get plenty of Air on job to clear chips and give occasional blast with WD40 or what ever you use for lube.

Every machine is different but with 3mm Carbide cutter at 1.5mm DOC you shouldn't have any trouble provided you clear chips. Just be ready on the Over ride buttons so can adjust Feed and Spindle speed on the Fly and you'll soon find the sweet spot for your machine.

Material Must be held down well and with thin material even more important so either Stick it down with tape or Screw down in several places before doing the profile cuts. If it moves or lifts you'll get chatter and with small cutters nailed on to snap.!!

[magicniner]

With copious air for chip clearance and no lube I have profile cut aluminium parts 20mm thick with hand sharpened budget 1/8" single flute carbide cutters so I doubt it's your cutters,

- Nick

[d4cnc]

Ok guys, thanks.
Yes, I think I underestimated the workpiece holding part.. At the moment, I've got 4 screws in the corners of the 400mmx200mm sheet and 2 screws in the middle. However, definitely will tape down in the future too.


I'll keep those settings for now then, change to coventional milling (I'm using climb) and do full 1.5mm doc tomorrow. (after securing it better)


I've got air on via a 24l compressor at about 30psi through 2x 1.5mm nossles directly blowing on the cutter, then a vaccuum cleaner connected right there too. No lube however.


So it's possible to get an ok finish on this aluminium?

[Boyan Silyavski]

Its like Dean says, you are rubbing it. Quite clear from the photo.

[JAZZCNC]

So it's possible to get an ok finish on this aluminium?

Yes no reason why can't get perfect finish but get your self can of WD40 and give cutter several squirts while cutting. It will help with finish and chip sticking.

Always Try to direct the air so it's blowing chips away from direction of cut otherwise you are blowing chips back into path of the cutter which get re-cut and this affects finish.

[sinnsvak]

I use a 6040 and my most used cutter is also 3mm single flute carbide. However, I turn it from 16000 to 18000 rpm around 300mm/min when I slot up to 3mm depth, and 400-500 mm/min when doing full depth (5-10mm) outside contours. I dont think the speeds you posted first would even work on my machine.

I also think a mister is necessary, I use alcohol because I also have a fan that draws the fumes outside.