PCB Trace Differential Pair Impedance
In this case, yes. 

In the very general case, there would be a difference that the twin 50 ohm line is ground referenced in the middle, whereas a true '100 ohm differential line' need not be. In some exotic RF components, the difference would be important.

For the case of differential data transmission, whether MIDI, SATA, LVDS, HDMI etc etc, the system will always be using twin anti-phase ground referenced transmitters, and twin 50 ohm line will work just fine.

Beware that a true 100 ohm diff line does not have any skew by definition. A pair of 50 ohm lines can easily have different physical lengths. They must be time matched to within a small period of the data being transmitted, easier with MIDI than 6GHz SATA. 

Time matching is easiest to accomplish if the traces actually run parallel and close to each other. You do not have to use either extreme of 'true 100 diff' or 'true widely-spaced twin 50 ohm' line. You can start with 50 ohm traces. When you bring them closely together, their impedance will drop slightly, which can be offset by narrowing the traces. Any PCB layout package worth its salt will have calculators to assist in the design of such a line for any specific substrate.

The system you are using should have a spec for the permissible skew. If it doesn't, then skew less than the risetime will probably be adequate.