No need for O flute for aluminum but you need a ZrN coated bit for best result. A two flute will also cut faster than one flute. The endmills from Carbide like the two flute 1/8in - 102Z are very good but you can get good ones from Drillman1 on EBay also. Use a F&S Calculator like the ones @Julien and @gmack have created to ensure you do not break or damage the bit trough overloading or feeding at the wrong speed.
If you need a baseline to start from for your feeds and speeds, I documented a similar usecase here (#102Z 1/8", profile cut in 0.08" thick 6061 aluminium)
I wouldn’t use a downcut or compression bit for cutting Al. Downcut endmills provide poor chip clearing and in aluminium that’s a sin. Compression only makes sense when cutting through a given thickness in one pass, and that’s not likely to be the case in metal. You can get away with any upcut carbide endmill, but ZrN coated are less likely to stick indeed. Spray some WD40 on the surface before the cut, and with correct feeds and speeds you should be fine.
hey guys checking the feeds and speeds. Looking at your example Julien. You used the formula:
“* to achieve the 0.0005” chipload at 12.000RPM with this 2-flute endmill, the feedrate needs to be 0.0005" x 2 flutes x 12000 RPM = 12ipm = 300mm/min"
For mine I purchased a 4 flute 1/8" ZRN endmill, so I have the 0.0005 x 4 flutes x 16,000 RPM (setting 1 on my dewalt) gives me 32 ipm
Going to keep the plunge at 4ipm, and keep the depth of cut the same as yours at .012"
Yes, your adjustement to take the 4 flutes into account and higher RPM is correct. However please note:
in the example I documented, I mentioned that I eventually used +50% feedrate override during the cut, because my 300mm/min was a tiny bit to slow for comfort. 450mm/min ended being better for my cut.
you will be using a 4-flute endmill, that will bring higher ridigity of the endmill, but also poorer chip evacuation, so if you are going to be slotting, keeping a small depth per pass sounds like a good idea (at 0.012" you should be fine). If you can use a little lubrication (drop of WD40) and/or a blast of air, that will put the odds of a good cut in your favor.
So what I would do if I were you is start the cut with those settings you mentioned, have your mouse over the feedrate override button, and increase up to +50% by increments of 10%. If it cuts fine (normal sound/vibration) at +50%, keep it there as it will lower chances of melting the aluminium.
EDIT: it seems to me that setting 1 on the Dewalt can just as well be 16500RPM, so you can easily round up that initial feedrate to 35ipm
Also keep your endmill stickout to a minimum. And do let us know how it goes !
Ok, all went well. As suggested , zrn endmill, sprayed the sheet with some wd40. Cheated it up to 130% speed. Kind of gnarly sounding when cutting metal compared to wood, but I suppose that’s to be expected.
Well it is a very nice piece, you are talented! I would love to take a look at the files but I have VCarve not Aspire. If you are willing to share, maybe you could also put on Cutrocket.
