Well your problem is largely a matter of experiments carried out in the past, and how they panned out.
I would use an Iscar insert mill because they are quite free-cutting. The shank is also massive all the way down to the tip, as opposed to a fluted mill with 3.5" of flutes. I would use the special grade of polished insert with sharp edges to assist with the free cutting action and chip flow.
I might use a shorter endmill to begin with until it has gone as deep as it can. It may work well at .125" DOC, maybe 125 ipm feedrate.
I would likely use a depth of cut of about .06" and 100 ipm feedrate for the 4" long roughing mill.
Its critical to allow the tool to sweep the corner to reduce the engagement angle. After roughing, I would plunge machine the corner radii within .005 of finish. This would be an effort to clear most of the material from the corner so that the finisher will not run into a big bite, where the engagement angle suddenly skyrockets. I would want to prevent a chatter pattern from starting, if at all possible.
For finishing, I guess there would be little option but to go with a solid carbide finisher. Probably knock the rpm down to 1200 rpm and maybe 25 ipm to try obtain silent cutting. Those corner radii are going to give you trouble with instant chatter if you use a 1" finisher. This is because the engagement angle of the tool suddenly rises to 90 degrees as the tool enters the corner. So I would beg the designer to permit a larger corner radius, say .525" If he won't hear of it, then maybe go with a smaller diameter finisher....25mm maybe or 7/8" if you could find one.