6061-T6 Facing finish

Hi All,

I’m trying to face some 6061 and I’m curious what sort of results I can expect out of the Nomad. I took a 3 thou pass with a Ti-Ni coated end mill. I’ve tried using the 1/8" dia one and a .25" one. Seems like no matter what I try with feeds and speeds and end mills I always end up with a bumpy surface finish. I can feel long ridges left after the cut (in the direction of the cut). Some parts of the piece are completely smooth. I’m wondering if I’m just up against the limit of the machine or if there’s something I can do about it.

Also, it sounded like the spindle motor kept loosing revs and then I’d see a visible mill scale where that happened. Not sure what’s going on there either. I’ll try to upload some pictures.

This was a .125 end mill at 8k RPM, 16 in/min with a 3 thou depth of cut and 50% step-over

No, you shouldn’t be. Those cutting parameters aren’t aggressive. Try a smaller stepover, maybe 35% and see what happens. Also, if you can, try adaptive milling (if you use Fusion 360) to keep a constant load, especially when you hit corners where the endmill engages more material.

1 Like

I’ve had really good luck with the spiral finish on aluminum in Fusion with both 1/8 and 1/16" square bits - very light machining marks which clean off nicely with 800+ grit paper.

1 Like

Thanks all! I figured it out, it seems like the secret sauce was not using a dull end mill and decreasing the stepover.


Always a good plan. I’ve just started using Zrn coated mills for aluminum as they tend to “pick-up” less material on the flutes. Re-ran an existing job with a new one of these (1/16" square) and the final surface finish was maybe 30% better than the same job before with a good, but used cutter. (Cutting 250mm/min, 10k rpm, 200mm/min lead in, 100mm/min plunge, 0.3mm optimal load, 1.5mm max stepdown).

Roughing with a 1/8" Zrn square, it seems like the cutter was just happier (compared to same job without the coated cutter). Without the coating, with fairly aggressive roughing, I always had this feeling that I was pushing the cutter too hard. (Cutting 380mm/min, 10k rpm, 250mm/min lead in, 195mm/min plunge, 1.27mm optimal load, 1.5mm max stepdown)

NOTE: I historically underestimated tool stick-out; with these small diameter cutters, it’s very important from a deflection and chatter standpoint. When mounting the cutter in the collet, stick that sucker as far into the spindle as you can get away with, even if that means the shank of the cutter stick out the collet on the other side (inside the spindle).

1 Like

HSS cutters may also give you a better finish than carbide. They’ll wear faster, but they are sharp! I think @Vince.Fab mentioned the same thing in one of his aluminum posts, and he spins a fair amount of aluminum.



This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.