we are getting through it but its taking a long tim.weve got 24 of them and each has 2.5 full days of work into them even running overnite. I have this op in the 5 axis now but even 5 axis doesn't help at this point. its only a .438 square so drilling the corners isn't even an option because the overlap so much. we are using Harvey long 1/4 in mills too.

No Bid!

Why no corner drill with the Flat Bottom? Just get a .250 Flat Bottom Drill from Harvey. I've held .001 with these tools. Just leave about 0.002 for finish. Speaking of Harvey, they have these tools with reach up to 20xD! http://www.harveytool.com/prod/Square-Miniature-End-Mills/Miniature-End-Mills/Browse-Our-Products_255/Miniature-End-Mills---Square---Long-Reach--Stub-Flute_92.aspx Nachi America has a fantastic Aqua Drill which could work. 120mm OAL, .250 diameter, 6mm shank. (You'd have about 0.720 to grip on...) Aqua EX Flat Long Shank. Series L9819. EDP: 1489290. http://www.nachiamerica.com/p-3/Cutting-Tools/Drills/AQUA-DRILL-EX-FLAT-OIL-HOLE-SERIES

Are you adjusting the feedrate for the tight arc motion? When swinging a tight arc, the OD of the tool is feeding around the arc at a much higher speed than the center of the tool. You may have programmed .0008" FPT, but swinging a really small arc will cause the OD of the tool to experience a much higher FPT (maybe up to .002"!!!)

^^^ EDM ONE AND DONE ^^ Makes life easy .

Then look to a dynamic process using the full flute of the endmill using a very small stpe over and slow speed and feed. Maybe 1000 rpm and .0005 to .001 per tooth feed rate stepping in .005 per pass. You said there is a .4 hole thru on the next part try drilling out the corners 1st then coming back and putting in the .400 hole is possible. Might be work hardening the material with the .400 hole. I suspect your going to have to have this Plunge EDM if the tolerance tight. Let me guess it was quoted to be done in 30 seconds and one endmill was going to last 1 million parts and the management is wondering why you can't make that happen?

Try plunge milling it stepping over a little bit at a time?