Tried to cut a divot tool (golf) from 1/8" aluminum with a 1/16" O flute bit (1/4" shank).
762 mm/min
0.1mm DOC
Was going really well and then the bit snapped.
Other than using a fatter bit, should I slow down the feed to like 500 mm/min? I kept it at 762 mm/min because I thought you had to keep a good pace going through aluminum to avoid the material overheating. Was I too aggressive or is this just not something a 1/16" bit can handle?
Pretty sure the metal that is filling in the lower left corner of the cut is the bit all chewed up. You can see it did successfully complete all passes on a few contours. It was probably done with ~30 of the 33 passes on the big contour it snapped on.
That’s a pretty good first try! Way better than my first try!
Looks like you ran into some chip evacuation problems. I wouldn’t have tried the 1/16 myself, but I’m a chicken. Looks like it was doing a great job, though. I’ve found on my 1/8 that much more than 1D deep, I need extra room. Try adding a roughing pass so you go around the shape twice on each pass, making the groove wider than the tool. Helps a lot on contouring/profiling. Takes about twice as long.
Alternatively, use a trochoidal/Adaptive path for the same reason. Takes 2-4 times as long, depending.
Or just use an 1/8 inch endmill on the 1/8 plate. That might clear it up too. What speed were you running the router?
Thanks for the info. I’ll give that a try once I get a new bit. Do you think the bit may have overheated too? I was thinking of breaking the code into 5-10 separate cuts and letting the bit and material rest for a while between cuts.
Looking at the product page for the bit, it suggests 16k-18k RPM which just feels too slow. But that looks like a red flag in my setup all of a sudden.
Probably ok. Did the aluminum get hot while you cut it? Mine generally doesn’t get over 105. I set my 611 to 2 for 1/8 tooling, which is about 18k rpms. That puts it in the 550-600 sfm range. I think I read that carbide is ok up to 900 for aluminum. We have plenty of power to go slower too. You’re using a smaller mill too, so you’re closer to 400sfm. So pretty good even for hss, but I’d let surface finish tell you whether to speed up. Your chip per tooth is already pretty good. I honestly wouldn’t change it.
Imo, after toolpath, the next thing to change is DOC. you can get back some of the time you lose on making two trips around the part by going a little deeper, maybe 0.11-0.13. Set up a few slot tool paths at various depths and try them out. 0.1mm is really not very much at all. I’m not saying you can double it with such a small tool, but even if you can add 0.01, it could save you a lap or two.
I didn’t touch the aluminum with hand - only with a paper towel to help wipe away some chips. Didn’t feel that warm from that vantage point but I can’t know for sure.
All great info, thanks again. Next try I’m going to try to increase my chip load with a slower RPM (maybe 2.5 or so to get it more aligned with your spindle speed) and add a roughing pass @ 1mm stepover. That stepover will cut part of the final pass with the roughing so should reduce the load on the bit during the final pass. Probably keep it at 0.1mm DOC for now (now I’m the chicken).
The color of the surface and the black looking chips makes it look almost like steel. I won’t insult you by suggesting you can’t tell the difference but it does look unusual to me.
I don’t know about dropping the speed, but it seems right to trust the data sheet. Those chips look pretty big, though. I wonder if you’ll have to go slower too?
When you add a roughing pass it should get calculated to the outside of the part, not along the finishing pass.
Or maybe you mean that you won’t need as wide a finishing pass? Then definitely. I’ve found that even when I only calculate a few thousandths for finish, I get bigger chips than I expect because the rough didn’t get as close as fusion expected.
Good luck!
So that is exactly why I think the bit melted off (not really, but overheated and then chewed itself up). The actual chips are very bright silver. You can kind of see it in the picture below and it should give you an idea of the actual chip size - pretty dusty looking, no?
But the material filling the contour in the lower left in the original post is definitely a darker material and the “chips” are a lot bigger which makes me believe it’s actually the bit in a gazillion pieces.
Ahhh. Looking at the picture you just posted, I think maybe those are reasonably sized, but you’re right :you can probably push it a little. You aren’t going to get big chips no matter what because the DOC is so small.
Any reason you choose a 1/16 mill? The 1/8 that Ryan sells are good quality and not a lot of money.
That’s a good reason! I just got a coated 1/16 kennametal for some steel practice and I haven’t even chucked it up yet because I just KNOW I’m gonna break it, lol.
