Re: [CAD_CAM_EDM_DRO] deep pocket milling

"Victor Cantu Jr." wrote:

> I have recently had to make a part that required a deep pocket in the center. The pocket was 2x3x3deep. I got the part done but, I wasn't satisfied with the chatter I got in the corners. the mat. was alluminum 60-61 . Does any one have any suggestions for me they would be greatly appreciated. thanks

One of the problems is in the corners the wraparound of the material increases, increasing
forces on the cutter dramatically. This is a major problem in deep pockets.
There are several solutions. Assuming you have CNC, you can program a
radius at the corners that is at least 25% greater than the radius of the actual
tool. This keeps the tool from suffering from the increased loading at the
corners. Something I have seen in some old McDonnell-Douglas boxes,
where everything is milled out of solid blocks of aluminum, is that they
would drill holes in the corners where the OD of the hole was slightly outside
the actual dimensions of the pocket. Then, when milling the pocket, the
cutter never actually went into the corner, and it stayed smooth.
This would be a trick when manually milling the pocket, and where the
extra semi-circular cut in the corners was not a problem for the design.

There is special tooling to solve this problem, of course. Where larger
corner radii are acceptable, you use a tool with a long, solid shank,
and a relatively short flute that is slightly larger than the shank.
Perhaps a tool with a 4" long 1/2" diameter shank and a 1/2" long,
9/16" cutter at the end. The extended shank tool is a lot stiffer
than the extended depth-of-cut tool. Solid carbide end mills are
AMAZINGLY stiffer than HSS! Also, within a particular material
and style, a 4-flute cutter is stiffer than a 2-flute. The disadvantage
is there is less chip removal space, so flood cooling or some other
arrangement for chip removal is a good thing.

Jon