Dry Aluminium Cutting Problem

I'm always having issues cutting aluminium on my mill. The side which is climb milled is not too bad, but the side which is conventional kind of grows a furr of re-cut aluminium.

The thing is, I have a reasonably decent vacuum above the cutter and I've tried all different feeds and speeds (have G-wizard).

What I notice is that the issue becomes far worse as cutting time goes on and the piece heats up. Does anyone think the heat of the aluminium could be an issue? It seems like it becomes 'sticky' when it gets hot and bungs up my cutter and chips don't extract well.

I tried a 2 flute cutter today and it seemed to work better than the 1 flute but then suddenly got cloged as in the picture below.

Has anyone else experienced similar? I realise coolant is the way to go, but I don't really want everything to be messy and wet! Maybe a mist spray would be a good middle ground.

Some pictures..

http://i608.photobucket.com/albums/t...k/DSCF9214.jpg
http://i608.photobucket.com/albums/t...k/DSCF9215.jpg
http://i608.photobucket.com/albums/t...k/DSCF9213.jpg

Below: This was extracted from the groove part way through cutting.
http://i608.photobucket.com/albums/t...k/DSCF9216.jpg
http://i608.photobucket.com/albums/t...k/DSCF9217.jpg

It's the heat build up in the part causing that. That's one of the reasons I switched to an aluminium bed and flood coolant, as they both help conduct the heat away.

Thanks Jonathan, I'm glad it's not a problem specific to me. I'll have to think about the best way to do flood coolant. I went with the HDPE bed specifically so I could use coolant, but I know it will be messy.

Could I ask people to post up or link details of their coolant set-ups to give me inspiration?

Quote:

---

Originally Posted by Tenson

but I know it will be messy.

---

It is.

Quote:

---

Originally Posted by Tenson

Could I ask people to post up or link details of their coolant set-ups to give me inspiration?

---

I don't think you'll find many people on this forum use flood coolant. My setup is merely a pond pump in a bucket, connected with some 16mm hose to the Z-axis upon which I've clamped a coolant hose to the spindle. There's a picture in my build log.

You might find that mist coolant would be enough to reduce the heat build up since although it clearly wont conduct much heat away, the coefficient of friction between the cutter and the material is reduced so less heat is produced to start with. Did you use any lubricant at all when cutting the part pictured?

Aluminium is a bitch for clogging up tools. Plenty of cutting oil and/or coolant is the only way to reduce it.

Quote:

---

Originally Posted by Tenson

Could I ask people to post up or link details of their coolant set-ups to give me inspiration?

---

Here's a pretty one I made for home use, had to pass wifely inspection.

One of those aluminium boxes with the O ring seal to make it weather proof. The lid is bolted to the end of the bed with a hole to drain the suds back in to the tank and type blue gasket compund so it doesn't drip.

In the bottom of the tank is a fibrous mat designed for filtering Koi carp pond water under a mesh to keep it in place. The oil goes down through that into a coffee machine pump I got on ebay. Spare pump on top of the tank. Then a hose to a magnetic nozzle.

I put it all together, switched on and found the pump was MUCH too powerful. Hence the knob at the back of the tank which allows most of the suds straight back into the tank.

I didn't use any oil at all. I've tried it in the past with WD40 and also water (not together) but it always gets whipped out the groove so fast! Even if I start out thinking I'll just use a tiny bit, the place gets flooded pretty soon. Yes the cut is much better, but I was under the impression dry milling was entirely possible.

I've ordered the bits to do flood milling. I just need to think about the best way to drain coolant from the bed.

I've also ordered a ripper mill so I bet that will extract chips better and not clog as much.

I got a bottle of this for coolant mixing - G/P Soluble Cutting Oil Coolant White Water 1 x 1 ltr | eBay

For dry cutting, you have to prevent the tool overheating so either add pauses to your program, or have a "dipping pot" of cutting oil on the bed which you return to after "x" time or take a rough cut first and no more than 0.1mm on the finishing cut. As you noted, climb milling always gives a better finish but may chatter more.

I cut aluminium dry all the time with just blown air and the odd squirt of WD40 and it's not a problem for me. I have mist and flood but both are messy. Flood obviously sprays every where and mist can be fumey depending on whats used. I only use them when finish is important but mostly I cut with just blown air.

What grade aluminium are you using because looking at those pics and the way it's grabbed and furred up it looks very much like the soft shity 1020 stuff you find in thinner sheets.
The grade of aluminium makes a massive difference and this soft stuff is like milling cheese strings and will defiantly need coolant.!

What size cutter, feeds/speeds and DOC are you using.?

Quote:

---

Originally Posted by JAZZCNC

I cut aluminium dry all the time with just blown air and the odd squirt of WD40 and it's not a problem for me.

---

That might be simply because Jazz chose the tool, chose the material, built the machine and set it up.

I get the same thing with my customers trying to connect USB, as soon as the computer realises I am on the other end of the phone it knows the jig is up and gives in gracefully.

You might think it is just "air and the odd squirt", but experience tells you when to blow and when to squirt :hysterical:

Quote:

---

Originally Posted by Robin Hewitt

You might think it is just "air and the odd squirt", but experience tells you when to blow and when to squirt :hysterical:

---

I find a syringe works well for this as you get better aim. Before I got the aluminium bed I would have to slow down for thin parts, or lots of parts at a time. I don't always use flood coolant with aluminium, as it does make such a mess and isn't worth it for a lot of things.

Shouldn't the chips be taking all the heat away?

I don't want the mess of flood coolant on my SX3 & have never had a problem by simply brushing parrafin onto the cutter & using a shop vac to evacuate the chips.

The only time I've had the material furring up on a cut edge like that is when the cutter's gone dull, which can happen quite rapidly.

I was using an oil based coolant and found it to be very sticky and it also created a lot of fumes. I have switched to Ultracut evo 250, mixed with water this stuff does a really good job without having to use loads of it. Aluminium can be sticky when it warms up and will clog up sharp tooling easily. The chips wont take all the heat away but should take away a good portion of it if your feed rate/spindle speed and DOC matched up.
You could try this: single flute 6mm cutter at around 700mm/min 12000rpm and 1.2mm DOC should give a good finish with a little coolant sprayed on and extraction to remove the chips from the cut.

I hate standing over the work trying to get WD40 on it. I just want to hit go and have it do the job for me :)

IIRC I was doing 1 mm passes. The 2 flute was at 1200mm/min and 14,000RPM. The single flute was at 650mm/min and 16,000RPM.

Yes I think the material is a soft type, it is only for cosmetic purposes and came on a Chinese product. I do get a similar problem with 6082, though to a lesser degree.

Quote:

---

Originally Posted by Robin Hewitt

That might be simply because Jazz chose the tool, chose the material, built the machine and set it up.

---

Yes some of that is true Robin. It's simple really I have the Chip load dialled in correct for my machine and the material I'm cutting which is mainly 6082-T6 or Ecocast.

I could tell my cutting conditions but that won't mean much and chances are they won't work for other machines. Each machine has it's own resonant frequency or sweet spot and finding it is harder than the mystical G spot.!! . . . But when you do it's nearly has satisfying just without all the effort. .:joker:

I think Often people(Which I ounce was.!) are scared to cut deep and the noise puts them off but often it's exactly because they are cutting too shallow they can't find the sweet spot regards resonance and chipload.!

Put some ear plugs in and try cutting deeper and see what happens.? You may get a shock at how deep you can go and the finish you achieve. I always use full depth 0.2mm finish pass when finish is important so the deep roughing pass often doesn't matter.

The key and secret to cutting anything is Chipload and when done properly the heat will leave with the Chip. The Odd squirt is just that one blast at start to put a light film on oil cutter and depending on length of Job then maybe one half way thru.!! I certainly don't stand watching, like now it's cutting and I'm in the house.
Another very important thing regards Aluminium in particular is chip clearing, you must limit chip re-cutting to absolute minimum other wise the tool will heat up from rubbing and pounding cut chips into material.

Hmm, I tired cutting thinner passes each time I had a problem as I thought it would create less heat. Perhaps I need to cut deeper. Chip extraction is obviously key too, but how do you do it well without coolant? I have a reasonable vaccum but a lot of the alu chips are too heavy to extract well that way. It works great for wood :)

What depth do you tend to do got the first pass, Jazz, and what tool do you like to use for general contouring? Do you use a ripper/rougher or a smooth flute?

P.S. Thanks for all your advice chaps!

Jazz,
what was the DOC and rpm for the G spot??????

Roughing endmills are only really useful when used with flood coolant, since the general idea is they make very small chips which are more easily washed away. You mentioned earlier 16000rpm at 650mm/min for a single flute cutter. If that's a 6mm cutter then the spindle speed is a bit fast, and setting the spindle speed too high does lead to excessive heat production. I use 12500-13000rpm with 6mm carbide cutters and 600mm/min for single flute, (almost) never more. The spindle speed is determined from the cutting speed of the material, so you will find the single flute and 2 flute carbide 6mm cutters require about the same spindle speed. As Jazz has said, using a finishing pass whereby you take off the full depth, 0.2mm wide, makes it fairly easy to get a good finish. Just make sure there isn't any residual swarf before starting the finishing pass. Whilst a lot of the heat can be extracted in the chips, on small parts like the one pictured they can still heat up if your bed has a very poor thermal conductivity, which is the case with HDPE.

Quote:

---

Originally Posted by Web Goblin

Jazz,
what was the DOC and rpm for the G spot??????

---

Wouldn't know It's a Fooooking myth doesn't exist. . :ghost:

Quote:

---

Originally Posted by Jonathan

Roughing endmills are only really useful when used with flood coolant, since the general idea is they make very small chips which are more easily washed away.

---

Not exactly true has I use 3 flute 8mm and 10mm carbide Rippers dry cutting 5 to 6mm DOC with no problem and can actually cut 100% diameter if required and the specs say upto 1.5x Diam full slot but my machine doesn't like handling that DOC so I keep it safe.
These rippers must have a finish pass has they leave a rippled/ridged surface, great for if you need a grippy surface like spindle mount holes.!!

Quote:

---

Originally Posted by Tenson

Hmm, I tired cutting thinner passes each time I had a problem as I thought it would create less heat. Perhaps I need to cut deeper. Chip extraction is obviously key too, but how do you do it well without coolant? I have a reasonable vaccum but a lot of the alu chips are too heavy to extract well that way. It works great for wood :)

What depth do you tend to do got the first pass, Jazz, and what tool do you like to use for general contouring? Do you use a ripper/rougher or a smooth flute?

P.S. Thanks for all your advice chaps!

---

Yes try cutting deeper but you must clear the chips.!

Blown air is the secret, Oh and having the machine vertical helps greatly. .:whistle:.!!
Vacuum has to be very strong but still doesn't clear enough, esp when slot cutting deep. Blown air is the only thing other than high pressure flood coolant that will clear the chips fully but again it's messy and you need a good or large compressor.
Either way your into mess and decent blown air setup with correct chip load gives just has good result has low pressure coolant because your not re-cutting chips which you still are with low pressure coolant. The best for tool life and finish is high pressure high flow coolant but for that you need a full enclosure or a Wet suit.!!
I prefer blown air has it's dry and don't have machine enclosed, the mess of dry chips I can deal with.!

Depending on Job I use ripper for hogging away material then finish with either HSS or carbide twin flute. I actually prefer HSS has it gives a better finish it's just wear out quicker but because I'm only often doing finish pass they last ok.
Some times I'll use Carbide on longer jobs for the full job if I'm being lazy and don't want to change tools.

I tend to cut between 2 to 2.5mm DOC for 6mm twin flute HSS often around 800mm/min 10-11,000rpm full slot. (Cutwell code E5521060)
6mm 2 flute Carbide between 2-3mm 900/1100mm/min 12-14,000rpm.
6mm 1 flute carbide 1-2mm 600/800mm/min 11-13,000rpm.
With the 8mm carbide ripper around 800-900mm/min 5-6mm DOC 8-10,000rpm (Cut well code E5711080)

I'm often adjusting the RPM and feeds on the fly depending on how the material is cutting and the load on spindle. I Don't really watch RPM and just monitor the Load on VFD and if it's getting too high then I know I'm being greedy. I never push the Load so high there's no overhead just in case hit any sticky spots or for when tool starts to wear.
After a while your ear will be your best tell to how well it's cutting but the VFD load is a good tool to watch.!

To give you some idea I never gum up cutters above 4mm and below that then I'm nervous has hell for both gumming and snapping so go OTT on the air and coolant.!! . . .But still rarely gum them up.!!

I disagree with Jazz, the 'G' spot is the little magnetic clasp on genuine alligator skin wallets that are stuffed full of paper £money. The sound that little clasp makes when it's released (& you can't describe it in words) makes wimmin go all wobbly at the knee's & make "Ooohhh" & Ahhh" sounds.

A gentleman will always carries a hanky to wipe the wetspots from her dribbling chin.

I do agree that the chips should be taking away most (if not all) of the heat. Every setup is differant & you need to experiment & perhaps overcome your hesitance to sacrifice a bit of material & maybe a few tools to find what works on yours.

Maybe:
your materail is crap.
feeds and speeds are wrong
your workholding is not great
your machine is not stiff enough.

I would:
thow that material into the bin (bin= return to china)
use a feeds and speeds calculator to get a good idea where to start
think about your cutting strategy....

Billythefish You do realise that this post is over 3 years old and the G spot has dried up long ago:joker:

Lol... Well I hope it may be useful for some future readers :-)