I'll take a stab, first, you don't say what size endmill your using, but I will assume a 3/16 and at 8000 rpms, your running close to 400 SFM, therefore, your endmill is fried. You didn't say what kind of stainless or condition, that shiny silver stuff comes in lots of different kinds. If its tubing assume it is 304.
Grab yourself a machinery handbook, Amazon is the cheapest at about $57.00, ebay has some older used ones, still just as good. In this book you will look up Surface footage, (Surface Feet per Minute). It will tell you that while milling, you are going way to fast. I would suggest with a HSS bit and 304, no more than about 50 SFM, this gives you (3.8/.1875) * 50 = about 1000rpms. I'm sure there is someone that can give you a better estimate, thats just a guess, but I think I'm pretty close. Now you have to think about your chipload. On a Cnc this is easy, on a maual machine its a bit more difficult, taking a full width cut is never a good thing, but on .035 thick wall, its not going to be too bad. Lets be conservative and say, .0005 per tooth on a 4 flute endmill, that gives .002 per rev. Multiply your 1000 RPM by .002" per rev and you get 2 inches per minute, now break that down into revoluttions of your handle and do the one mississsippi two mississippi thing to try and keep an even chip load. Now if your running in 304, keep that sucker cool, you say you flood the part with cutting fluid, now does that mean flood coolant, or you are just pouring a bunch of oily stuff on it before you start cutting, the bunch of oily stuff won't really keep the heat out, it will help, but you might be better just holding an air nozzel on it while cutting.
As far as the fixture, the functionality seems pretty good, the main thing is that it is made out of plastic. One thing that you will learn and may already have and don't know it, is that rigidity is key. Think about it, your using a benchtop mill, which is not the most rigid thing going, and then you have a plastic fixture, the endmill, HSS(not very rigid in itself) pushing off of one side of the slot and pulling itself into the other, now the spindle and machine flex, say .001" and then since cutting metal isn't the easiest thing to do, the fixture moves another .002". So all of a sudden, you've gone 2 revolutions without cutting anything, and then all of a sudden your cutter, with all the forces you've built up from the deflection, starts to cut and you have a .003 chip load on one tooth that you decided should only be taking .0005", this results in one roasted endmill and one unhappy machinist.
As far as endmills go, I like carbide, but on a smaller machine that bounces around a bit, its probably not the best idea. I would get a 1/4" cobalt rougher, and then finish with a 3/16 cobalt finisher.