I tried milling a small hole (about 1/8) in 1/4” aluminum but only managed to snap endmills. (Lucky they’re cheap) I used Fusion 360 and helical ramping into hole. I tried slow, fast and really slow. All snapped at various times. Has anyone here managed to do this? If so, what speeds and feeds did you use?
I've done 5mm holes with a 1/8" carbide o-flute endmill. Circular CAM, DOC 0.1 mm, Plunge Feed 250mm / min, Linear feed 750mm / min, 15,000 rpm on my Bosch Colt. Circular machining does not ramp into the hole, it pecks at it (plunge, cut, withdraw 2mm, repeat) so I'd keep your DOC shallow. I've come to the conclusion that small circular holes should probably be drilled, not milled.
1) Do you really need to use 1/16" endmills? That is probably close to impossible to learn on. The smaller the endmill the more on the money everything needs to be. 2) You have to go slow. You want to do a bore operation, and set the pitch to something crazy small like .05mm.
I use 1/8" center drill bits for holes that must be 1/8" they are cheap and work well, something like these, I can't find the ones I have, but they are nothing special. Set them up as a separate operation and peck drill the holes. Gary
I need to create a 3.3mm hole for tapping. My initial idea was to use a carbide spot drill to create a dimple and finish it on the drill press. However, when I did that the entire z axis flexed and didn’t leave me convinced. (Perhaps I need a better quality one, used 90deg carbide spot drill from eBay) So then I tried with the 1/16 since it was what I had on hand. One idea to try is to use a 1/8 end mill and plunge about 1-2mm, enough to let the drill register against the top of the hole. @Gary Caruso, what rpm/federate do you use? My router only goes down to 10k. Any other suggestions?
do not drill with an endmill. they are just not good at it. always ramp in (as you are). circular interpolation will work, aka 'helical bore', medium feed, high rpm, low depth of cut you will need some kerosene(1) to keep the chips from sticking to the bit, that is probably what is breaking them. also, the smaller the endmill, the fewer flutes it should have. so for 1/16 one would prefer a single flute. this makes sure there is space for the chips to evacuate (1) or a cutting lubricant made for aluminum. I am cheap so I use kero.
1/8" is about 3.17mm. I think it's close enough to 3.3mm for your tap to cut the thread in the aluminum so drilling will be the best solution. It's always the best solution in small diameter holes.
I tried the helical cutting but to me it seems like 1/16 is just too delicate to handle this on my machine. While I’m not thrilled about plunging with the endmill I am prepared to try it since they’re cheap and I only need to create 12 small pockets. I’ve been weary about chucking a drill in the router but maybe 1/8 is small enough to run at 10k So my options at this point are: 1. Plunge 1/8 endmill about 1.5mm, finish on the drill-press. 2. Try with my 135(?) deg spot still, finish on drill press. 3. Try to drill with 1/8 drill and drill to final size on the press. I think I will do some tests with these techniques.
Did you follow my link to the super cheap short flute drills? These type are commonly used for drilling rivet holes in aluminum. They have a tip like a twist drill bit but short flutes so much stiffer than a long standard drill bit.
I ordered some now. I’ll give them a try and see how it works out. I’m concerned that all drilling might prove to deflect my Z too much.
Short and slow drill pecks and you should be good. I was able to drill the holes for M4 threads and my linear rail bolts lined up nice, with an OX. Cheers Gary
I tested using my 120 deg spot drill and to plunge a 2mm pocket. Both resulted in significant deflection in Z. I also tried plunge with very low feedrate (125mm/m, 5 IPM). Still flexy... I have some 1/8 drills in the mail that I will try but I'm not getting my hopes up. I think I might just have to accept the flex. All the holes may be offset 0.05-0.1mm along Y. However, this is actually not a critical measurement for this project. Another option would be to lay them out manually and punch them on the drill press. Not sure that this would be more accurate. At least I learned something new about the machine. I've always considered the Z plate of the Sphinx to be stiff enough to not flex. Well, I'm not so sure any more. While pulling on the router I managed to flex the plate about 0.05-0.1 mm in the middle. This distance will be amplified by the distance between the router mount and the bit, resulting in flex 2-3 times that at the bit. I'm actually considering going back to the hose-clamp + angle bracket mount I used in the beginning. This might actually be superior to having a (single) openbuilds style router bracket. The router is attached in two places along Z and it is also closer to the plate resulting in less leverage for the forces.
I've used my minimill to mark holes by cutting a 0.5mm deep "hole" with a V bit - basically using the mill as a center punch. Then, I just drilled them with the drill press. Works great and everything winds up in the correct place. I haven't found that approach to be beneficial on softer materials like plexi, HDPE or wood, but it sure helps on aluminum.
I tried drilling with the 1/8th drills and the flex was about the same as the other approaches (which I expected). The finished hole also seemed to have a lot of slop in it. I could insert an 1/8 endmill and jiggle a lot... So, I'll probably go with spotting the small holes ever so slightly with a spot drill and using the drill press to drill them out.
I've had good luck with 2-flute 3/32" end mills for making 3mm holes in aluminum. I also use helical ramp in F360 making these holes as pocket cuts. I've only done 1/8" thick aluminum, but I don't know why thicker would be a problem. I use a Makita set on 1.5 for speed (~12000), 762mm/min feed, 0.3mm DOC.
