Recently purchased a Shapeoko 3 XXL with 2.2kW water cooled spindle. My most immediate need is to machine some 6061 Al. I was browsing the wiki but didn’t see 6061 listed with any in depth machining specs. Does anyone have any recommendations? I purchased a pair of High-Performance Carbide Two Flute End Mill, Square-End, TiAlN Coated, 1/8" Mill Diameter, 2" Overall Length, 0.75" LoC, with my total cut depth being around 0.75" in the Al.
I do a LOT of machining in aluminum, (95% for the last 3 years, up until my latest wood project).
First: Cutters: ZrN Coated cutters are a must.
Second: Lube: I recommend my WD40 drip system for finish cuts
Third: Air Blast (I recommend a cheap mist sprayer from eBay ($11) and just use it for air. Need to get those chips out of there
Forth: Tighten EVERYTHNG
Fifth: DOC and feeds, (This is what I like to recommend) 0.015 DOC at 15 IPM, then start increasing it by 0.005 and another 5 IPM, until it starts to make too much chatter/noise. Every machine/set up is a little different…find YOUR sweet spot.
Sixth: I like 10k to 15k rpm, spindle speed. Some wild and crazy guys (Vince) like a LOT more speed, but his machine is (now) heavily modified
This is the norm…
I LOVE Fusion 360 Adaptive cutting, and that is a whole new ballgame and not something for you to start with.
What CAD/CAM software are you using? As @RichCournoyer said, Adaptive toolpaths are what you want to be using as much as possible, they let you remove much more material without pushing the rigidity requirements of the machine too far.
Have a look at This thread at whats possible with this machine and Adaptive toolpaths.
For now I’m just setup in the Carbide softwares. I design in Solidworks and Creo, I’m an Advanced Manufacturing engineer so I have a pretty strong knowledge of CAD/CAM packages. Is there a recommended CAM for the Shapeoko?
Griff
(Well crap, my hypometric precursor device is blown…)
7
A lot of us use Fusion360 for CAD&CAM. Lots of support, informal, here and on line.
~6% optimal load? That seems like it’s really low at that point and your MRR is suffering. You could reduce your DOC and increase your OL to get a higher MRR.
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…
