You can certainly get away with milling steps in soft jaws and holding it in a vise. However, you will need to be pretty consistent with vise pressure, and knowing when you're over tightening or under tightening. When holding onto a plate, depending on thickness and width (in this case 1/8" thick, 3 inches wide which is not too bad), it tends to bow up and away from the vise and it acts like a spring or drum skin. The cutter will put additional upward force on the material, plus vibrations, and will probably harmonize. One way of eliminating this is cutting a dovetail relief at the bottom of the jaws so that it is only contacting and squeezing the part at the top.
That being said, the best, most reliable, most fool-proof way to hold sheet stock is in a fixture with toe clamps or toggle clamps giving top pressure, and there is a lot of good advice already given for that way. For locating, you can machine "bump stops" in a plate to push the material against in the y and x directions (be sure to relieve the corner), or drill and ream 3 pins for locating, 2 pins on the back side and one pin on the left side is usually my setup.
As for endmills, it's hard to make a recommendation without knowing your machine better. I believe the Tormachs have a fog buster, and not flood coolant, which makes me want to steer you away from carbide, which tends to chip when it overheats. But I've seen plenty of people using carbide in that system without problem. Supermill makes a great endmill, as does destiny tool. Harvey tool also is really high quality and tend to last longer in my experience. I would suggest using 2 flutes, as it is more forgiving, and there is more room for the chip to evacuate. You're not going to be able to keep up with an extra flute in my opinion and the amount of time you will save is negligible. And if you are interpolating, consider the following formula: ipm x (hole diameter - tool diameter)/hole diameter = programmed ipm. So for a 2 flute 1/16" endmill you'd be going 10000rpm x .0015 cpt x 2 flutes = 30ipm when cutting. But to interpolate a 1/8" hole, you'd program it to go 15 ipm to maintain that .0015 cpt. Good luck