If it were me, I would think along these lines:
- it seems you only want to do a profile cut, so you do not really care about which endmill diameter to choose => then go for the largest one in your list, which is the 1/8" 102Z. The larger, the less likely to break if you get feeds & speeds slightly wrong. Also, at 1/8" you do not really have to care about runout, while at 1/16" and 1/32", it could be a problem.
- Winston’s example is using the #122Z, which is 1/32" and has 2 flutes. He is using 10.000RPM, 152mm/min, so the chipload for his cut is 152/(2x10.000) = 0.0076mm
- I consider that acceptable chipload can be increased roughly linearly with endmill diameter, which would translate to four times that value for a 1/8" cutter, 4 x 0.0076mm = 0.03mm. On the other hand, my personal chipload reference err on the side of caution at 0.0005"/0.0127mm for a 1/8" in aluminium. So I would probably pick a value somewhere in between, say 0.02mm
- assuming you have a Makita and can actually use 10.000RPM, that chipload would translate to a required feedrate of 0.02mm x 2 flutes x 10.000 RPM = 400mm/min (which happens to be exactly the value mentionned in on one of the two entries in the wiki section for copper that Will references, though RPM is not stated).
- depth of cut now: Winston used 0.006" / 0.15mm for the 1/32" endmill, so 20% of the endmill diameter. With your 1/8" #102Z, 20% would be 0.025" / 0.635mm. That sounds a bit too much to be comfortable for me (I tend to limit DOC to 10% of endmill diameter in metals), so I would just stick with 0.15mm: it does not matter because you are not aiming at reducing your cutting time anyway by taking less passes. Shallower = less risk of breakage. 0.3mm would most probably work just as fine.
So that would be: #102Z, 10.000RPM, 400mm/min (~16ipm), DOC 0.006"/0.15mm. Plus, as Winston said, clean-up the chips during the job (vacuuming, blowing air, using a brush, whatever).
And finally, when you start the job, if you do not see nice tiny chips of copper flying, the endmill is probably melting/pushing material rather than cutting, and you should probably stop immediately, and reconsider the settings.
BUT, I am not at home so I would ideally also verify what G-wizard calculator has to say (and plug in the right copper type in there too), and TEST this myself before answering (I remember I did profile cuts in 1 mm copper a few months back, I would need to look up my settings), so take all of this with a grain of salt, I’m sure others with jump in to correct me if needed.
Also, what feeds and speeds does CarbideCreate come up with for this situation (102Z, copper) ?
If this is not urgent, I’ll test this over the week-end, I’m interested in the exercise to consolidate/correct my feeds & speeds approach/guidelines anyway. Just need to find where I stored my copper…