CNC Feeds & Speeds Course
Join 50,000+ CNC'ers! Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:
- Our Big List of over 200 CNC Tips and Techniques
- Our Free GCode Programming Basics Course
- And more!
Issues cutting aluminium
Im just getting started and got my mill up and running this weekend. Its a Skyfire CNC (the small one, but still about 160 kilos) with a 24k rpm spindle.
Since its fairly rigid and I got servos I figured I should have no problems cutting aluminium. But it has been a nightmare. To date I have managed to gum up 3 different cutters and straight out snap one of them.
This is how I have set up my workflow, first I have entered the tool data in G-wizard to get the speeds and feeds, then I use those values to plug them into Fusion 360 using adaptive 2d clearing to get a constant engagement toolpath and then post the code from there and load it into Mach3.
Depth of cut and cut width are pure guesses on my part, so I started with an in my mind conservative figure of 2mm cut width and 1mm depth of cut. After some trial and error I found a combination that worked where I had a nice and steady stream of aluminium chips.
The settings where as follows: 24k rpm, 5mm 2 flute carbide end mill (unnamed Chinese, slightly dull), 3560mm/min feed, chipload was 0,0296 mm/tooth, surface speed 377 meters/min. For this setup I used the HSM box and light rough setting.
For cooling I used alcohol, by spraying the surface prior to starting I had a light layer all over. Surface finish was great and you could barely feel the toolmarks with the fingers, very smooth.
Here is a picture of that operation, chips where coming off in a steady stream and no smoke from the alcohol, it did not even evaporate so things where obviously cool. The gray streamers on the picture are chips, they where cool and not producing any smoke either.
Since that seemed to go well we figured we could increase the cut depth, I dont want to use only the tip of the tool. So we doubled it and increased the setting to rough. This gave a similar feed of 3510 mm/min out of G-Wizard. plugged those figures into Fusion 360 and again using the same adaptive code I tried again. The cutter was doing just fine for one layer, (area about 40x80mm) and then on the second layer it suddenly gummed up. It took me a second or two to stop the mill and it managed to run about 10 centimeters leaving a weld like build up in its wake. It did not break though so I figured it was because it was dull to begin with. (due to input pin error in Mach3 spindle control I ran the spindle backwards with it when setting up the machine…)
After clearing off the aluminium and realizing it was dull I switched to my other cutter of the same model, this one was sharp and completely fresh. I jogged it over the build up to remove the ridges etc and then I restarted the same program. After cutting some air for two laps it instantly snapped on the first corner where it was actually in contact with the material. I assume this was since I came in at full speed? This was only the built up aluminium ridge left after the last cutter and a very small engagement so I was really surprised that it just broke off.
Next cutter I tried was a 3 flute DOHRE carbide aluminium cutter. It says 3F-5X13X6X50LX45 HSC 500a on it, looks like its dimensions followed by the model.
Since I was running out of tools I figured Id be more conservative with this one, so I reduced the cut width to 1mm and the depth of cut to 1mm. I also remember reading that it should have a surface speed of 250m/min on the webpage where I bought it. So I entered the tool data in G-Wizard and entered the max surface speed. Since G-Wizard did not change anything based on that and kept the 377 I had used with the 2 flute mill I lowered my max spindle speed until I had 250m/min. I also lowered the setting to finish. This resulted in the following settings:
You can see the result below, almost immediate gumming and a raised ridge along the edge where it was cutting. Unfortunately my phones camery is shit and I also removed the aluminium build up from the cutter before taking the picture, but all three edges was completely gummed up. You can also see where I managed to stop it to the left of the red circle.
The finish on the side here is done by my 2 flute using the 1mm depth of cut and 2mm cut width settings described above. It is silk smoth and you cannot feel the tool marks so Im happy with that.
But, I obviously need help to move forward. Ill start by ordering some more 2 flute cutters, but any help would be very appreciated. First question is, can I still use the above cutter? It feels sharp to the touch and I managed to remove all the aluminium. If someone can point me in the right direction so I can use the cutter before I get some new ones that would also be highly appreciated.
I will also order a fogbuster and a compressor but for now Im stuck using spray by hand coolant, just so you know.
Also note, I use metric measurements, I can ofc convert from American measurements, but all my settings are metric in these pictures.
- Leo Sandström asked 9 months ago
- last edited 9 months ago
Any time you get that “gumming up” effect with aluminum, it’s a coolant lubricant problem. Not enough coolant is reaching the tool or the coolant being used is not a good enough lubricant. While I know Datron uses a particular kind of alcohol as lubricant, this is with very high speed spindles and I have no idea what rules they encourage for that use case.
The other thing I notice in this case is you’re not doing anything to clear the chips, so they’re recutting. That’s another invitation for chip welding. You must both provide adequate lubricant and adequate chip clearing. In fact, be very paranoid about the chip clearing and you will see your results improve.
The Fogbuster with a decent water-soluble coolant will be the answer.
Hi Bob, and thanks for the reply!
Im not sure I understand, I have seen plenty of examples of people running aluminium dry, so there must be a way for me to do it as well. I can understand if my particular alloy is one of the gummier ones, but my two flute mill was shooting a steady stream of chips in the 8 o clock direction when the cutter was engaged from the 1 to 3 o clock position looking from above in the direction of the cut. Under that circumstance I cannot see recutting occuring too much since it was just shooting the chips away consistently.
I can also understand if the geometry of the much more expensive aluminium 3 flute cutter is somehow dependant on coolant to cut well, but it would surprise me if that was the only way to do it. In my mind the sweetspot is probably smaller, but it should be there. Now the question is, when gumming, do I increase rpm, decrease it? Increase/decrease chip load? I was honestly hoping for some tips along the lines of what to try first.
I have just tried both higher and lower rpm with the 3 flute, but to be honest, no matter what I do with it the cut is not clean. So I just switched to my slightly dull 1 flute cutter, it has a much higher angle on the flute and I have been able to make a steady stream of chips leaving a clean surface. Will experiment some more…
- Leo, while I know you want to cut aluminum dry, and you’ve seen some people succeed with it, it’s just not the right way to do it in most cases. Aluminum actually has a chemical affinity for your cutter’s carbide that causes it to weld to the cutting edge. There are conditions that will minimize the effect, and there are tool coatings that can protect the tool, but these both have serious limitations. Coatings are thin, and as soon as the coating wears through the aluminum will bond to that spot and you’ll break the cutter almost instantly. You may be able to live with that, just be sure to get the right coatings and replace the tools before the coating wears out. The conditions that minimize the problem have little to do with feeds and speeds and everything to do with keeping the chips away from the cutter. You’ll have to make extremely shallow cuts and use compressed air or vacuum to remove the chips as soon as they’re created. This works best in cases such as foam board laminated to a very thin aluminum sheet. Cutting a thick block of aluminum this way is bound to fail if the cutter ever gets down too deep in a slot or pocket and the chips build up. Another approach would be to try exclusively using HSS tooling which has less affinity for aluminum. All of this is working way to hard to fix a problem that is easily fixed. All it takes is a mister and the problem goes away. You don’t have to run flood coolant at all.
- You must login to post comments
Managed to get things working with my old one flute mill, 1mm depth of cut, 20k rpm, 1300mm/min feed, cut width 2mm andd 0,035mm/tooth chipload.
This seemed to work better than 10k rpm with similar chipload since more chips flew off the workpiece leaving almost nothing to be recut.
However, the special and quite expensive 3 flute aluminium cutter is still a no go, simply cant get it to give me a clean cut on any speed…