Sure! I guess I have done enough where I can add some potentially helpful tips
For aluminum, my limiting factor is certainly the Bosch 1617 EVS router I'm using. It's been great for what it can do and runs like a champ, but it cannot mill aluminum in the recommended ways per many YouTube videos. It doesn't have the rigidity to do 3D Adaptive clearing by coming in from the side of the piece and controlling the optimal load which the more advanced spindles seem to perform with ease. I often see online depth of cuts in the 1/4" to 1/2" depth range but controlling the optimal load - no way with this router. Accordingly, I just decided to go shallow and accept the long milling times per piece. I run it at it's top speed setting of 6.
I'm referencing Fusion 360 CAM. As a starting point, I use 0.02" DOC, 50 IPM, and an optimal load or stepover resulting in 1/2 the bit diameter cutting. I have used 1/2" bits, but I now try to keep my max bit size at 0.25". If it's roughing I'll set it to "both ways" and for finish cuts its a climb cut or "left". Adaptive clearing is important as trying to 2D contour results in too much of a load and goes bad quickly. Lack of chip evacuation and the bit getting gummed up happens fast! So I'm often milling the entire aluminum stock except for what is remaining for the finished piece. I don't cut anything out of aluminum like you can with wood. Which makes using dowels and such to rotate pieces for two sided milling a challenge. So I milled a fixture plate with dowel holes and such to secure wood / 3D printed jigs to help accurately locate and flip pieces. Also posted elsewhere on here about setting up the depth probe to locate the X and Y 0,0 as well which has been helpful with aluminum.
I'll typically face the rough aluminum to final depth and use a micrometer to check. I'll clamp in my milling vice or use the painters tape / CA glue trick to secure. The CA glue trick is a Godsend! If I tape and glue, I'll run the facing operation on the waste board first to ensure a flat surface. So in Fusion, I typically copy / paste the same part a few times and copy / paste the set up. Reason being, my first set up is with the stock at initial depth, second set up is after facing it to final depth. I try to chamfer any and all edges. If you run 3D adaptive with the chamfers on the model it will try and mill the chamfers. You can use the 2D Chamfer on the model hard edges but that only works on 2D. I'm often chamfering 3D edges, so I use a 0.25" bull nose bit and 3D Scallop routine to accomplish that. There is a Fusion 360 tutorial on how to do that online somewhere. The settings are not obvious but it works. So that's a reason for multiple copies of the same model. Sometimes I'll add patches to ensure the Adaptive and Parallel routines don't deal with the holes / etc.
I may increase the depth of cut to 0.025" but never above 0.03" - so no mater what I'm doing it can take several hours to mill one side of a piece. The logic is this will dull the bits sooner, so I use cheaper SpeTool bits from Amazon. I think a pack of 5 bits at 0.25" two flute is $40. They work well for this application. Haven't had a dulling issue yet. But when that happens they are cheap to replace.
In general, I try to make the 3D adaptive work with a 0.025" maximum roughing step down and an optimal load of 0.1. This essentially uses about half of the bit diameter (0.25" bit for example) and takes a very shallow pass. I use a feed rate of 50-60 IPM. I'll leave 0.005" of material on the Radial Stock for a climb cut finish pass - typically a 2D contour with a step down of 0.5 inches. I try not to use Pocket Clearing as it engages to bit too much early on - there's a lot of discussion online about Adaptive vs Pocket.
For smaller holes, I'll use a 1/8" end mill. If you read about aluminum milling a single flute is recommended but they can be harder to find / more expensive so I pretty much have 2 flute flat endmills. As an example, for my 1/4"-28 holes I'll use a 15 IPM speed on a 2D contour, but I'll set the "ramp" to ensure it takes less than 0.01" per revolution. Essentially ramping all the way down through the hole. Maybe even more like 0.005" per revolution. It's slow but effective. Compressed air for chip removal is a must. I don't have any attachments so I just keep my air compressor handy and blow air on it about twice per turn. Metal chips go everywhere as I am not using an enclosure, so it's just some vacuuming time when I'm all done. No big deal. I don't trust my enclosure vacuum set up to effectively remove chips from small / deep holes and aluminum can gum up and go real bad really quickly with the wrong settings / conditions.
For larger holes / maybe a 0.25" bit at 30 IPM. Again, adjust the ramp angle to keep the amount of material removed per revolution to 0.008" or something close to that. I just eyeball it now on the Fusion preview. If cutting the exterior of the hole leaves material in the center, I'll often sketch a smaller circle and use the sketched object to first remove the inner material then finish with the actual hole contour. I just find ramping a 2D Contour an easy and surefire way to mill holes in aluminum. If I have to run two routines per hole that's fine with me.
For all holes I'll leave 0.005" material and clean that up with a finish pass climb cut. I'll typically make the rough cuts climb cut as well for the holes.
So it's slow, but so much better than me trying to accurately use a drill press and such
I'm on a tapping spree, so I try to ensure the tap hole is deep enough for 6 threads from the screw. I've read any more than 6 threads engaged doesn't increase the holding strength. Loctite and threaded holes in aluminum seem to be plenty strong for my purposes. Inserting McMaster-Carr parts helps with this evaluation.
I'm not using any lubricant - so all dry cuts. I want those chips out and away from the cutting area. I'll run a finish pass with a Parallel routine using a 0.25" bull nose bit at a stepover of 0.0125" - this takes a while to complete, but results in a nice pattern and I don't need to sand or do other finish work. I'm not a patient enough man to enjoy sanding and finishing aluminum. So I let the machine do it. The finish from dry milling / facing is OK, but nowhere near as nice as a professional job with lubricant. So the parallel with the BN bit is a good second place alternative for me.
Chamfers - typically 25 - 30 IPM and a Chamfer width and Tip Offset of 0.02" each. Fusion defaults to 0.04 but I think that's too big for my purposes. This is with a 90 degree V bit. That's for the 2D Chamfer CAM routine. Anything in 3D needs to use the Scallop trick mentioned above.
Tolerances - space between my object walls and the jig walls as an example - typically 0.5 mm. Don't ask me why I switch to metric, I just seem to have an easier time remembering 0.5 mm for spacing.
But since everything online I looked into is Imperial for CAM I stick with that.
For smaller bits - I bought some end mills from Kodiak Cutting Tools. I've gotten as small as 0.078" diameter. They had a close out sale on 4 flute micro endmills which is about 3 flutes too many, but with keeping such shallow cuts it doesn't have a negative impact. Same slow speeds / small incremental depths on the ramps, and lots of compressed air. Bit I'm able to cut some nice small holes and such.
Lastly - sound! Milling aluminum is very noisy and its obvious when something is wrong! It will sound awful and you'll need to hit the kill stich quickly and turn off the router quickly. I may not hover over the machine, but I'm always within ear shot of it as best I can. Since parts take a lot of time per my methods, I always try to have something else to do while the machine is milling.