With the track and gap parameters you have, you won't get 100 ohms differential impedance with any standard (if any at all) core / prepreg thicknesses.
You will need to make the gap much less and widen the traces somewhat. I don't use less than 4 thou track widths due to the fact that a minor etching issue can introduce errors that are a large percentage of the track width.
Some numbers that work:
Track width 4 thou, track separation 4 thou, depth to plane 6 thou on 1 oz copper gets you pretty close according to the Saturn PCB toolkit.
These are all pretty standard values for PCB design.
Notes on coupling.
Tightly coupled pairs (within a pair) are quite common and this has the advantage of having a somewhat higher single ended impedance on a per track basis within a differential pair which is often easier to implement. 100 ohm differential pairs that are tightly coupled have a typical single ended impedance of around 65 ohms.
Loosely coupled pairs have a single ended impedance of half the differential impedance.
This coupling is not the same as pair to pair coupling (where a decent gap is required).
There are a lot of values that would work, and a great deal depends on the specifics of the core / prepreg material used by the vendors as the dielectric constants for prepreg (in particular) varies widely by manufacturer. If I ask 3 PCB vendors for suggested geometries I will usually get 3 different answers.