Thread: Dry Aluminium Cutting Problem
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.
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. .
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!
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.
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.!!
Blown air is the secret, Oh and having the machine vertical helps greatly. ..!!
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.!!
Last edited by JAZZCNC; 29-01-2013 at 09:12 PM.
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.
By Bush Flyer in forum Metalwork DiscussionReplies: 55Last Post: 13-05-2016, 09:57 AM
By Pointy in forum Metalwork DiscussionReplies: 5Last Post: 05-05-2014, 09:59 AM
By steeplejack in forum Marketplace DiscussionReplies: 3Last Post: 19-10-2013, 10:52 PM
By stewpid22 in forum Projects, Jobs & RequestsReplies: 0Last Post: 21-09-2012, 01:11 PM
By kylelnsn in forum Items WantedReplies: 5Last Post: 09-08-2012, 09:54 PM