I, also, would run it with a 1/8" endmill. It may not be that much slower than a drill cycle, since it can be done in a continuous operation, The power requirement is less than for drilling, and peck drilling requires a lot of dead time for the retract/re-enter.
As for a drill, screw machine drills are shorter than standard (jobber length) drills. In 1/4", typical is about 2-1/2" overall (63mm) with about 1" (25mm) gripable shank. They can be shortened by regrind, if needed. I would not suggest shortening the shank. You want enough for good hold without the collet touching the flutes. If you regrind to shorten it, you need to use a decent drill grinder tht can do a proper split point (Drill Dr might be good enough, with care, but I would definitely take a lot of care. The swing attachment for a bench grinder are not gonna do it) or the balance will be off. At several thousand (or over 10000) RPM, this is a bad thing.
MSC, McMaster-Carr, and pretty much any other industrial supply have these in all of the expected flavours and toppings (HSS, Cobalt, carbide, TiN coated, TiAlN coated, etc)
General drilling info (with MDF, based on more research and only a little experience at high speeds, and the way that metals and plastics behave. Take this with the appropriate grain of salt)
If you choose to drill, note the chip thickness, as well as chip load. (feed per rev-- Feed rate and RPM determine this-- and peck cycle parameters) Too low a chip thickness will lead to rubbing and destroy a bit fast. At 10000RPM (low end on a Shapeoko), the cutting speed is 190m/min(625ft/min), and a feed rate of 250mm/min (10IPM) gives a chip of 0.012mm (0.0005). This is a real high speed and a light chip for an HSS 1/4" bit, even in MDF, but other flavours will be ok at this speed with a higher feed to bring the chip to about 0.05mm (0.002") or even 0.1mm (0.004") (1 to 2m/min (40 to 80IPM) at 10000RPM). I have not seen much from the bit manufacturers, but there is a fair bit of discussion on line (for example, the mastercam forum: https://www.emastercam.com/forums/topic/72025-cnc-drilling-into-1-thick-mdf-with-332-drill-bit/ ). Basicly, you don’t want to rub through or make fine dust. You want to drill such that you get chips that will clear via the flutes.