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 (http://www.mycncuk.com/threads/7248-Save-my-sanity-1050-grade-aluminium?p=58776#post58776) 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!


18105

[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.

[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 ;)

18116

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 :encouragement:

[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!
1812918130

[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?

[d4cnc]

Yes, the new aluminium sheet I'm going to cut, I'm planning on lining up some of the holes perfectly with the T-slots to screw into.. I was trying to avoid just screwing straight into the spoilboard with wood screws as I thought it would quickly get spoiled.. but I've since cut a 200mm pocket 1.5mm deep into it (set the bed for Z0 rather than the Z-1.5mm I wanted) and now dowsed it with lubricant.. so I think that plan is out the window.

I did find this interesting though.. http://www.cnczone.com/forums/diy-cnc-router-table-machines/155514-mdf-oil.html
So maybe I'll swap out the Draper lubricant I have for a can of WD40.. and just hope for the best.

[lucan07]

I need to come up with a solution for not destroying the MDF board with lubrication..

I always seal MDF with a couple of coats of Rustins MDF sealer a little oil or WD40 not a problem and great preparation if you want to paint or varnish.

[d4cnc]

I have a lot of Rustins MDF sealer here actually.. I was just a little worried about applying it and the MDF swelling.. then needing to resurface it and undoing the work of the sealer by taking off the top layer.. I guess if I apply a few coats, it'll seep in a lot and then when I resurface it, I'll still have a good layer of protection. It's probably worth it for the T-slots alone anyway.

[lucan07]

I find little swelling if any when dry if any maybe the edges which I always soak well, even then when dry I cannot see your bed needing more than a tickle to re true, it should certainly be less than wd40 or water.

[Clive S]

but I've since cut a 200mm pocket 1.5mm deep into it (set the bed for Z0 rather than the Z-1.5mm I wanted)You could make the pocket a little deeper and wider and then make a plug to go in it and glue it in position and re skim the bed.

[d4cnc]

If I wanted to use a 2mm cutter or even a 1mm cutter (obviously after a lot more practice as I'm sure I'd break them just by looking at them at this stage), how would that affect things? Presumably, the smaller the bit, the slower the feed.. and higher the spindle speed? It would be nice to get some tighter inside radiuses. (radii?)



You could make the pocket a little deeper and wider and then make a plug to go in it and glue it in position and re skim the bed.

Awesome idea! Thanks for the tip!

[Davek0974]

Possibly try
2mm, 1.5mm DOC, slotting, single flute, 24,000rpm, 120mm/min
1mm, 0.5mm DOC, slotting, single flute, 24,000rpm, 54mm/min

I have not gone that low yet though;)

[d4cnc]

Many thanks again. I've not been brave enough yet to try the 2mm cuts but will do later.. (I want some 2.2mm holes)


When it comes to work holding the sheet of aluminium and taping it down with carpet tape, what does everyone do with the protective backing?
Does that become the top as you cut through it? While the otherside is stuck down?
Or do you stick the carpet tape to the protective backing side ?
Or do you remove the protective backing altogther?

[Davek0974]

I always remove the film on both sides, the top layer gets in the way of the coolant/air i've found.

[JAZZCNC]

When it comes to work holding the sheet of aluminium and taping it down with carpet tape, what does everyone do with the protective backing?


On the lower side I leave film on if in good condition as it makes getting the tape off easier. On top surface then I tend to take it.

[d4cnc]

After a little experiment, I settled on sticking it on the film on the underside too. Worked great! Stuck strong. Easy to remove from MDF & aluminium. I used the Dial brand one from B&Q..

I tried the 2mm cutter on the settings above on some 2.2mm holes, and all seemed ok. I used a steeper angle helix this time and the chips certainly do fly like that!

I just did 1 pass.. am I right in thinking that due to this, the accuracy isn't great?
eg. some holes I can fit a 2.2mm drill bit in nicely.. others are too tight..
If I wanted it more accurate and repeatable, I'd have to pocket the holes at Ø2mm and then do a contour finish pass to enlarge to exactly 2.2mm?

[Davek0974]

Generally yes, a roughing pass leaving 0.1mm or so then a finish pass is best, i find it works well.