My first attempt at cutting aluminium highlighted the need for a lubricant. Though i might have gotten away with it if my cutter had been new and I'd kept the cut depth shallower. My criteria are: low mess, low smell, non-toxic, no special equipment needed, and environmentally friendly. But it has to work well too of course! So this thread is for recommendations and discussion of lubricants for light aluminium cutting on a small CNC router machine like an ox or workbee. I've seen all sorts of recommendations: dedicated lubricants (often with unknown ingredients) , WD40, kerosene, motor oil, beeswax. I really like the idea of using beeswax as long as it actually works well enough. I have plenty on hand, and it would meet all my other criteria.
Kool Mist 77 is very good, no-toxic, etc. You will need to mist it, but a mister can be bought for $20 on ebay, and then just need to hook it to a compressor. Kool Mist 77 | Kool Mist Coolant | LittleMachineShop
You really shouldn't need coolant for aluminum. Welding chips to the bit just means you are cutting too slow with too many RPMs or too much DOC making too much heat. Slotting will always be tough with these soft machines. Coolant can make the chips glob up (re-cutting chips is bad) , constant air blast helps. O-Flute bits work great. Trochoidal or "adaptive" type HSM machining helps a lot. If anybody has a successful recipe please share. Cheers Gary
I wasn't regarding it as coolant, but as lubricant, preventing heat rather than dispersing it - and helping the chips to release rather than sticking them together. It also seems to me that if the chips glob up then the lubricant is too thick or too much. Choosing a lubricant that avoids that is part of what I'm interested in finding out here. that said, yes, in hindsight after checking G-wizard my first attempt was slotting too deep and with too much deflection and a bit that may have been damaged when I started. G-wizard wanted to go slower and with higher rpm though so it wasn't that. But then what would I know I'm just starting - nevertheless loads of people do recommend a lubricant for aluminium.
The thing is that there are so many variables involved. Spindle speed, flutes, coating, speed of cut, depth of cut, machine rigidity, etc. Maybe tell us more about your setup.
rub a wax candle over the surface and on the bit before cutting and use HSM techniques for the cuts, especially slots. obviously we cannot cut so deep but the method works very well on light machines.
screwdriven workbee, makita 700 router. Bought for wood carving, but of course now I have it I'm thinking of loads of aluminium parts I would like to make. Mostly just cutting out shapes and cutting odd shaped holes in approx 2mm aluminium sheet. I figure there are lots of people with similar machines who probably didn't buy the machine for aluminium but nevertheless want to do it sometimes.
right I get the idea, and I will try it. For cutting out the outside of a part out of a sheet, how much bigger than the tool should the slot be to be effective? Should I try this with a 3/16 slot and a 1/8 mill? removing 50% more material than a straight slot - I can see it's easier on the tool and would help with chip removal but it's also more cutting in total. If I'm cutting out the outline where's the sweet spot in terms of removing more material than I need to vs making the cut easier? is this beneficial on wood too, or not worth it?
For 2mm aluminum you should be able to slot cut with a good tool, the ones I use are $4 , for over 6mm I could not get anything to work slotting, and had to use trochoidal tool path, But i'm also belts and not screws. My trochoidal setup; -width is +50% so it's 4.5mm wide for a 3mm tool -4.5% of tool dia trochoidal step over (3mm o-flute) -1000mm/min X & Y and 400mm/min Z axis -RPM is 4 to 4.5 on the Makita, for a two flute go slower.. (i just noticed 4.5 comes up a bunch this is coincidence... or is it!!) -3.3mm depth of cut, have done 6.6mm (one pass on 1/4") but chip evacuation is less automatic. With these settings I can set it up press play and walk away.. the chips are completely thrown from the slot and no welding. I slot cut 19mm (0.73") baltic birch plywood with a 4mm two flute at 1200mm/min 3mm pass/ so ~six passes, could push harder I think, a 3-4 on the Makita, adjust by sound, if it sounds like it's bogging speed it up. Cheers Gary
IIRC my settings on the failed aluminium cut were 3mm 2 flute up cut 600mm/m about 2 on the makita. (12-15000rpm??) 0.4mm depth of cut It still seems to me this should have worked even if not ideal. it's not totally out of bounds on G-wizard. BUT I had too much stickout, and I may have previously damaged the tool getting it out of the collet. I know I chipped it further up which isn't relevant to this cut, but maybe I had damaged the tip as well. it got to the third pass on an outline profile slot before it became obvious it was getting too hot and was struggling because of chip welding. I bought the makita rather than a spindle because it is straightforward and quiet at the slowest speed, I didn't anticipate having to use the faster speeds so much... looks like that may have been a mistake and I'm in for putting up with the noise for a while. is that a 4mm upcut you are using for slotting ply? does it tearout much? I have bought some cheap solid carbide cutters from ebay so I can not have to worry about destroying them as I learn. all this is useful advice for me, but it isn't about lubricants. I was hoping there might be some info out there on which lubricants are suitable for what and why, more detailed than just "use type X".
If I remember correctly David the swarfer once said, here in this forum, that heating oil (or diesel fuel) are good lubricant for cutting aluminum.
Once again, my suggestion doesn't have anything to do with lubricant. But Gary Caruso's post above I think hits the nail on the head. Too many rpms and/or two slow feed and/or too much DOC. I have tried trichoidal milling, but have yet to have much luck with it. What has worked for me is slotting like you are, with a 2-flute 3/32" (2.38mm) bit, <12000 rpm (about 1.5 on my Makita), 762mm/min feed rate, and a 0.3mm DOC. Since you are using a larger bit, the cutting tip would be moving faster at same rpm. With that and a slower feed rate and deeper cut, you will be "rubbing" metal more without cutting (creating heat). I suggest reducing DOC, lowering rpms and/or increasing feed rate and see how it goes. From what I read, the "sweet spot" for aluminum is pretty narrow. One additional thing I will be trying soon is to put an air blast on my bit. I got a compressor and one of those cheap nozzles on Amazon. (It will also allow misting, but I will try just the air blast first.)
I've done a considerable amount of aluminum cutting and the settings I used were along these lines: 3.175mm 2 Flute 24,000 RPM 635mm/min .5mm Depth of Cut I do use air to blow the chips out of the way, chip clearing is key, as well as a solid workholding setup.
these last two posts seem like contradictory advice to me. CNCMD - your settings are very close to what i did except for the rpm. Your settings are consistent with G-wizard recommendations. Scotty - isn't that very high chipload you have on those numbers? I haven't run it on G-wizard yet, but it seems like a fast feed and slow rpm. my bits have arrived so i'll try again soon, when I get some time. does anyone have a table of speeds correlated to numbers on the Makita? It hadn't anticipated the difficulty with knowing what rpm I'm actually using.
Is it possible to create a sufficiently focused suction to suck the chips out of the way and avoid blowing them all over the shop? I realise it is more difficult to create than an air blast.
Good info guys.. Just shows how many variables there are, what works for one might weld chips for another! Some more tips; -I get much better surface with Climb cutting vs conventional.. which should be expected on aluminum. -Use 6061 or other "easier" to machine aluminum alloys. -If you have the slightest welded aluminum on the endmill it will lead to more and more! and if you can't pick it off, use some liquid drain clog remover (or sodium hydroxide aka Lye) dip the endmill in some for a few minutes and it takes the aluminum right off, leaves the carbide unharmed, might get slight gunmetal grey coloration but that's ok. Cheers.. Finally Friday
Climb cutting should be used, I second that. My recommendation would be to do some test cuts, start off with .20-.25mm doc. I can tell you that a vacuum will only do so much, and gets pretty time consuming standing there the entire time. Yes it does make a mess to blow the chips but it does work well in my opinion.
I was wondering about a narrow nozzle - maybe 10mm at the tip, very close to the bit and attached to the router clamp - that could be used to push air in either direction, as an alternative to a dust shoe. like a 3D printer blower but with the option of suction...
Well there is only one way to know for sure. Many guys 3d print a piece that sits on the collet and acts as a fan. I will see if I can find a link.
Nice thing with the O-flute is they fling the chips out so well, I've been doing hour long cuts with no assistance or babysitting in 1/4" 6061. I just looked at the chart and a 4 on the makita is 22000 RPM's but that's with a single flute. these are the O-flutes I have used the 2 and 3mm with success
Page 5 of the owners manual. https://cdn.makitatools.com/apps/cm...b3-3b81-48d3-b5c1-3ae0fe4e121d_RT0701C_IM.pdf
Hi Craig. Good Post! You know what I'm going to ask, if it isn't already there, can you put a copy of this in the Resources area. Cheers Gray
hmm, pretty sure I didn't get an actual manual with useful info like that. I never realised it was missing.
I tried a standard two flute today and with a finish pass, really happy with the results, this was still torchoidal, then a 300mm/min 2.2mm doc finish pass at %5 bit dia, 3 on the Makita. My machine just isn't ridged enough to slot aluminum.
that looks encouraging what software are you using to create a trochoidal profile path? did you use a lubricant? what do you consider a "standard two flute"? spiral upcut? straight flute? what length of cutting edge?
Yes, Estlcam No lube Spiral up cut $5 link provided Climb cutting and 300mm/min, 5% finish cut (5% of dia finish pass) I did one today at 400mm/min and it’s not as nice as that one. It’s so picky!!
