I appreciate the feedback - it was suggested to try a lighter OL to get the deeper DOC. I did find that it had a little bit of chatter, but resulted in nice chips (I am a sucker for big chips)
I had not actually calculated any MRR until now - and you’re right on the money, 1mm OL * 2.4mm DOC gives me a significant’y higher MRR than the figures I quoted above, in fact close to 50% higher MRR…
Milling aluminium is a pretty new thing for me, I’m quite comfortable doing it but still working out what the best OL & DOC are for my machine
Right, try that out. I also have seen a lot about having a chipload around 0.0254mm when cutting aluminum. I assume you are using a 3-flute endmilll, which results in a chipload around 0.0223. If you bump that to 0.0254mm, you’ll gain bigger chips and another 14% MRR. Your spindle should be able to handle since my Dewalt router can.
Yeah ok, I’ve been running 24,000rpm, 1600mm/min feed with a 2 flute endmill. This gives me 0.033 chipload according to F360. As mentioned earlier I’ve settled at 1mm OL, 2.4mm DOC at these speeds and it seems to be going ok. Any suggestions?
I haven’t had the opportunity to do a lot of testing lately, I’ve been busy making timber parts for family, but I will get some time in the next few weeks to do some good testing.
Thanks for the clarification on the 2-flutes. That sounds great and like you know what you’re doing. Glad I could help. It just comes down to testing now.
Do those feeds and speeds sound similar to what you’re running? My machine is stock
My testing will be stepping up DOC in 1mm steps, then OL in 0.1 steps as follows
1mm DOC - 0.3mm OL
1mmDOC - 0.4mm OL
and repeat until I get chatter
then
2mm DOC - 0.3mm OL
2mm DOC - 0.4mm OL
repeat until chatter
And carry on until I find the highest MRR without chatter. Not sure if anyone else has done similar (I’d be interested in those results if they have) but it’ll be good to do it on my setup.
All the Aluminium I have is 5083, which I think is a bit softer than 6061
These machines run G code so pretty much any software should work as long as there is a grbl post processor.
One thing to remember with running less than 50% radial width of cut, is chip thinning. Fusion does not account for this with the exception of 2d facing if I’m correct.
These calcs are great to find actual chip thickness and mrr, plus recommendations.
Unless the machine has mods, imo, 0.100 is plenty deep for adaptive docs. And I try to push at least a 30 thou opt to take the heat away. There are also certain ways to setup part and toolpath orientations to maximize ridgidity in the cut directions. Little more advanced and every machine is different.
As far as testing cut formulas goes…Richard is right on the money. No surprise there
For adaptive - start with 0.001 chipload minimum and a light doc. Increase feed and router speed until you are comfortable, then start increasing the doc. There are also times where huge depth of cuts aren’t the most efficient. The most important thing is being smart with chipload.
Most of the time i’ll find the limits of my cutter and back off 15%. If you are chasing maximum metal removal then use a three flute, if you want reliability use a single.
Hi Rich, like Alex I’m a total newbie but I’m planning aluminum jobs already, nothing extreme, just simple cuts (contour) on 1/4" sheets. I have already ordered ZrN bits form C3D and can setup aircooling at some point. My concern is I have a DW611 and the slowest it can spin is 16K rpm. Is that too fast to start on alu? Obviously I will adjust feedrate accordingly, something like 20 IPM…thanks for the recommendations guys, really helpful. Forgot to add, I have an XXL so probably not the strongest frame…but I’ll cutting small parts (like 4"X4" max)
I would think working in one of the XXL machine’s corners (front left or front right most likely) would help, at least slightly, with frame deflection.
Used correctly, imo you are probably not going to get the point at which the frame extrusions deflect or bend any significant amount.
Especially on a stock machine, cutting forces shouldn’t exceed a few pounds. The vast majority of the deflection comes from the X/Z delrin wheel sets. Imo the absolute most important thing on an XL or XXl is to make sure the center of the wasteboard doesn’t sag and is well supported.
Rpm by itself is just a number, feed by itself is just a number. Combined they are important (plus flute count) and give you chipload. Create cam around the chiploads your machine can take, start with minimum 0.001 for 1/4 and up, 0.0008 for smaller . On a bone stock machine I rarely could feed fast enough to go above 24,000 (0.250 endmill), ridgidity limited.
Dont be afraid of using your rpm, just know that if you feed too slow that you’ll clog and break cutters.
Well, the Makita is only $99…(or $72 for a recon. on eBay…I bought a back up there).
I have two concerns, the XXL is not as rigid as the S3…just a matter of physics due to its extra length so the DeWalt WILL work, but it’ll make more noise and could start some chatter (harmonics) that could shorten the life of your cutters…so at some point you may ask yourself…how many $20 cutter do you want to damage before you spend the $72 for a Makita…just saying…
Ok guys, thanks for the recommendations, I agree the XXL will flex more. @Vince.Fab : I have already added support to the bottom center of the wasteboard to limit sag. @Rich: Yeah I should have gone with the Makita instead…
Anyhow, Winston Moy recently posted a C3D video about cutting alu on a XL (with some recommended feeds and speeds). The machine seems to be doing well with the 102-Z endmill @ 10k rpm and 20IPM (which if I’m correct is a pretty decent chip load=0.008). He says that scaling the feedrate up 60% (for use with a DeWalt) works but it’s less forgiving for the endmill in case of mistakes. I think I will try some cuts with the dewalt @ 16k rpm and 30 IPM see how it goes, my work will be mostly plywood/wood and some alu but if things go well I will make more and more shiny stuff and I don’t want to waste endmills!
Looks like the 102 is an 1/8 2 flute. That at 10k/20ipm is 0.001 chipload per tooth.
Even carbide create aluminum defaults call for 15k rpm/60ipm which translates to a 0.002 chipload. To be on the absolute low end on 16krpm you should run at least 35ipm.
@Vince.Fab Ok that’s the feedrate I had in mind for a first trial with the 102-Z. I’ll get the endmills next week so I’ll give a try then and let you guys know how that goes.
You’re not wrong… I just cut some 6061 for the first time and it cut like butter… I could still manage a decent finish on the 5083 but 6061 is certainly easier to get that finish, can probably push a lot harder on the bit without it melting the material too.
Can anyone recommend settings for a 1/4" end mill? I’m running a 2.2kW spindle and I’m currently setup for 1/4". I have a few slabs of 1" thick 6061 I’d like to mill.
For an example of what my goal is: I have a few sheets of 24"x24"x1" 6061 that I’m cutting discs from. 4.5" OD by 3.5" ID. Would moving to Fusion360 or Mach3 be the way to go here? 1/4" end mill with adaptive clearing? Maybe follow the 4.2mm DoC, .4mm OL, 1600mm/min @24k as recommended above?
As far as software goes:
If you’re doing big aluminium jobs I personally think Fusion360 is the way to go, those adaptive toolpaths work well with the shapeoko, and give you a lot of flexibility
Mach3 is control software, which won’t work with a carbide motion board, unless you’ve upgraded/changed your board then CarbideMotion/UGS/CNCJS will be fine for F360 Toolpaths
Have you done much aluminium machining? @RichCournoyer gave some excellent advice in the second post of this thread
I use similar to the settings you mentioned but only go around 2.5mm DOC. I’m sure it can be pushed harder but I get good results with those settings.
There is loads of great info earlier in this thread from Rich and @Vince.Fab, also in this one , I suggest re-reading the whole lot then starting out conservative and working your way up until you find the limit, then back off 10%
