Calculating differential PCB traces - Edge-Coupled Microstrip
It appears that I should solve for odd characteristic impedances of 50 Ohms each. Is this true?


Yes, the differential-mode impedance is equal to twice the odd-mode impedance (at least for symmetric geometries).


  My board house can do 5/5 mil trace/space. Is there any reason not to use these values?


If you can fit a design with larger gaps and wider traces, then the differential impedance will be less sensitive to over-etching or under-etching during pcb fabrication.


  How much of an effect will soldermask have on the circuit? Should I keep the differential traces uncovered?


Is a fairly small effect. But if you can, it's worth checking the geometry with a simulator that can account for the effect. Your fab shop may be able to do this for you, if they aren't a totally low-cost shop.

Leaving the traces unmasked is also an option. But remember to leave a sliver of solder mask around each component pad to act as a solder dam.

If you are using a higher-end fab shop, you can also simply specify that you want 100-ohm differential traces, and let them adjust the trace width according to their knowledge of the material characteristics, solder mask thickness, trace thickness, etc.