Yet Another Post Regarding Aluminum

Ok so I’ve spent the last few days really trying to perfect my feeds speeds and tooling for cutting aluminum.

I’ve just been trying to make a pretty simple hold down clamp (pictured below). I’ve got one that’s really close to the nominal dimensions, only being a max of .012" off, and I didn’t go through with the finishing passes so it may have been better, who knows. Either way I’m happy holding .012". I achieved this via a trochoidal strategy, buuuut it took over 40 minutes for that specific one. I could’ve pushed it slightly harder I think (was 1mm DoC @ 1200 mm/m iirc) as it wasn’t struggling. Also worth mentioning this was a single flute end mill I got from Ryan’s store.

I took that good one to work and let the big boy Haas and Tormach machinists take a look at it too see what they thought. I was told that with that specific finish on the side I was recutting chips. I was then given another 1/8" endmill to try, but one with 3 flutes. I originally tried to use that with another trochoidal strategy that was slightly more aggressive. That didn’t end up working out due to insufficient chip clearing, and I got lucky and welded a chip to the bit. Even more so lucky it wasn’t too hard to get it out :P.

My next plan was to try the 3 flute with a more generic strategy plus using a mister with air or with coolant to make sure chips stayed out of the cutting path. .5mm DoC, 750mm/m feedrate. I tried coolant, but decided to not use that until I can really dial in the mister because it took a ton of air pressure to draw it out and it was just too much that it started to fog up the garage. So for the rest of my attempts up until now, I’m using the mister just for air to help blow out any chips while I’m standing there with a vacuum getting what I can. As far as the pushing the machine’s limits goes, this setup seemed to work pretty well as long as I kept chips out. I read on CNC cookbook that this is pretty much the #1 thing to look out for when cutting aluminum with a machine like ours. Was also down to about 8 minutes total cutting time, and at first it seemed like I could even bump it up faster. Until I looked at tolerances…My .375" slot went from like .368" on the first part to like .425", and the ends of the slot were out of round (also pictured below). My OD was also like .050" small on both sides.

Up until then I was just using a riser on my main MDF bed to get as high up on the Z axis as possible, which I of course faced. Then held down a 12x12 .250" aluminum 6061-T6 plate to it. I waterjet 6061 at work often and it’s normally never bowed (so it’s my favorite material to cut lol) so I was pretty annoyed when my plate was bowed. I ended up getting a drill press vice, and some machinist parallels in hopes to switch over to 6061 flat bar which should be more…flat. I also hoped this would help this problem with the terrible tolerances since with parallels I can get it pretty damn close to the center. Nope. Same problem. I did, however, get it slightly better by slowing it down to 500mm/m. Slot seemed rounded but was still too big. Ironically it seems to be better on the machine if I run it faster. Less chatter mostly, if any. I also tried a brand new 2 flute end mill and my single flute end mill with this program.

Is conventional milling just that bad on these machines? I would just hate to have something take 20+ minutes if I can push it harder. Especially when I go to work and can see the same thing and more done in barely a minute lol. I’m also not sure if this is something that can be helped by having coolant misted on it as it’s going. I don’t think that it’s a power to the stepper problem, otherwise the slot would be undersized, and I’m pretty sure my belts are pretty well off too.

Ooo yay an aluminum post :smiley: I like these threads cause aluminum is pretty much all I do right now. Can’t really relate with the laser guys :frowning:

You are very right about chip clearing. I just set up my air blast nozzle on the gantry and I am buying my compressor later today (it is 1:27am in California hehe)

You are using a dw660 right? I suggest you take off the locking feature at the bottom. It allows some of the internal cooling fan’s air to blow some of the chips away. It has a circlip that is pretty hard to take off unless you have the actual tool which I didn’t. It also makes it look cooler and makes getting to the collect a little easier. By no means is this a replacement for a proper air blast, but it does help significantly and it’s free.

About your tolerances, .425" actual and .375" nominal? Woah there, something tells me your gcode was off there. I can tell you for certain that assuming your gcode is spot on, your slots will always come out undersized due to deflection in the machine. Perhaps you entered the wrong tool diameter? If you used the same gcode but w/ a different bit that is very strange.

I don’t know why I see people conventional milling D: It’s no good for aluminum! You will read just about anywhere that climb is better because it leaves a better surface finish and reduces cutter pressure. Everything they say is true, especially with trochoidal milling strategies. The only downside to climb milling is that it can increase deflection because the cut begins at full width while conventional eases into the cut tangentially.

With trochidal, you can really push the depths. I can cut 1/4" plate in 1 pass. More depth increases the “efficiency” a lot. When cutting a slot, always increase the depth before the stepover/step length. I get this sweet sound of no chatter, but the sound of the dw660 being slowed and loaded. That is a very good sign, because it shows you’re using more HP efficiency but not overdoing your hand on your machines rigidity.

Looking at that piece I would instead pocket the whole thing instead of making a trochoidal rim around it. There’s a certain size where the savings are minimal. Besides, no tabs, less cleanup!

Make sure your belts are nice and tight. It is better to have them too tight than too lose in my opinion. Too tight and they eat away at your stepper power, but too loose and the whole machine just gets down right sloppy.

I’ll be sure to take off the collett cover, I can’t stand using it to tighten tools so I guess that’s a win win. I should’ve also made myself a bit more clear when I said conventional, I just meant using a straight cut along the inside instead of trochoidal. I’m not actually sure how to make sure it’s set to climb milling in Estlcam, or if that’s possible. Maybe I need to try to quit being intimidated by fusion’s CAM side and maybe that would solve my gcode problem too? I had also thought it was a gcode error so I re cam’d it on a different computer, same result.

Kevin is the master at aluminum right now, have a look at his videos.

A few things I noticed, try a single flute. Takes less power to cut with as there are half the cutting faces of a two flute…three flutes is a no go in my opinion, we use a high rpm spindle. Twice as much time to get chips out before the cutting blade comes back around as compared to a 2 flute bit, 66% more time compared to a 3 flute (that’s why you got welding)

A straight slot is going to get bigger than your intended dimensions as the bit vibrates from hitting both sides and you have very little control, Tricoidal or adaptive is key, no straight slots in metal.

Move slower and cut deeper, use more of your bit so you don’t have to throw them away as often.

Most important. Use a finishing pass, never on any material try to cut to dimensions on your first pass. Do the dirty roughing work, then come back with a nice light finishing pass and watch those dimensions tighten right up.


Hmm, I feel like I’ve been setting up finishing passes in Estlcam incorrectly. I’ve tried doing so, but in running, it only seems to finish maybe PART of the slot, then it just ends the program. The way I’ve been setting it up is doing my normal CAM options, depth, machining order, then for finishing tool I usually select a replica of the same tool, minus the trochoidal step length, so trochoidal is just disabled. Don’t know if I should be selecting the same tool or not. Using the default finishing allowance, so it should set it to 5% of the tool diameter. Hopefully I’m doing this right.

Kevin, what speed are you able to get away with by taking a 1/4" cut? I’m interested in trying this, and before I was going to attempt an 1/8" cut but if you can do 1/4" I’d rather do that too obviously lol.

I would do something like a 0.4mm finishing offset, the rest seems correct. 0.1mm isn’t enough.

Alright I’ll give that a go and see how it works out.

About the offset, I agree but don’t at the same time. The offset is assuming that the roughing pass is exactly the (overall dimension-the offset). The thing is, due to deflection in the machine as I said earlier, your pockets, especially roughing, will always come out undersized. Because of this the offset doesn’t need to be that high, because the finishing pass should be rather light and adding a high offset will worsen your tolerance because your cut width is high = deflection.

Just did a test cut with my air blast, and I was .2mm under/oversized. I set the offset to .05mm (pretty much nothing). May try .1 or .15mm
This is just for aluminum though due to how hard it is compared to wood. In wood, no doubt a bigger offset makes more sense.