[dkaustin]

My first efforts at machining 3D contours in 6061 aluminum are encouraging, but it's clear I have a long way to go. Using an 1/8" ball mill with a very small stepover, I'm getting decent results, but the surface is striated in the direction of the tool travel. I'm assuming this is because the axial point on the tip of the ball has essentially zero rotational velocity.

Would I get better results using a square-end mill with radiused corners, or is there something obvious I'm overlooking?

Thanks in advance for any guidance.

[holbieone]

what do you mean by "striated in the direction of the tool travel"

I'm assuming you making rough and finish passes

you can use a flat bottom end mill with or with out corner radius it all depends on the direction of cut and can that cut be made with out the back of the tool clipping the surface

you will get a better surface finish with the larger radius of a flat bottom end mill

[Andre' B]

One technique I have seen used on really high end mills is to tip the part so the flat surfaces are at an angle to the ball end mill. That way you stay away from the very tip as much as possible.
The other advantage you get is you keep all three axis moving all the time and so avoid the stick slip problems.
Downside is it makes programming and setups more complicated.


It works on high end machines with backlash as close to zero as money can get, and you can get a mirror or very close to it, finish right off the machine.
Not sure if it would be as effective on a hobby level mill.

[zephyr9900]

dkaustin, use a good-quality carbide endmill. I use Atrax, which are usually on sale at reasonable prices from Enco. Use the shortest flute length that will reach the deepest part of your contour (i.e. clear any vertical or near-vertical sections of your contour,) and likewise "choke up" as far as possible on the shank of the endmill so there is no excess overhang when reaching the deepest part. Stiffness is the name of the game. You want to minimize the deflection of your endmill. Carbide is a stiffer material than HSS, and the deflection of a cantilever beam (which essentially what an endmill is) goes up as the cube of its length.

When I really want a nice contoured surface, I do a "semi-finishing" step. In my tool table I define a phantom ball-end mill that is .010" larger in diameter (i.e. .005" on the radius) and .005" longer than the ball-end mill that I will actually be doing the contouring with. My tool 8 (actual endmill) is .250" diameter and 4.805" long. My tool 10 (phantom endmill) is .260" diameter and 4.810" long.

I generate a finishing process in MeshCAM using tool 10, and when I actually machine it with tool 8, it leaves a uniform .005" thick "shell" all over my part. Then I generate and run a finishing process with actual tool 8, and its load across the part is more constant, minimizing any variable deflection of its tip.

Best regards,

Randy