You can do that, or you can call the diff pairs out as width and spacing. Really however you communicate well with your shop is fine. Even better if you call them at the start of your design to work on the stackup with them. Nobody knows their process like they do. It could be easier/cheaper for you to make a minor change that you wouldn't know about otherwise.
Also I'd say you should be specing your dielectric thicknesses and your over all board thickness. The shop will likely slightly adjust your widths based on what they know about their etching and lamination process.
That's another part of the Stackup that is nice to work with your shop on ahead of time.
The calculation looks correct, but the tracks are too wide.
For example, a single 0.75 mm track on a 0.36 mm substrate, has an impedance to ground, unbalanced, of about 49 ohms. Thus a "differential pair" any long distance apart will have an impedance of 98 ohms, without any coupling between the lines, i.e. infinite mutual impedance. It only takes a tiny bit of mutual impedance to bring the differential impedance down to 90, which is why your package puts them so far apart.
Hence the warning about spacing/height. You don't really have a differential pair, you have two single-ended lines, which as you say isn't ideal for rejection of coupled interference, or reduction of radiation.
A differential pair should have a significant mutual impedance, at least similar to or smaller than the impedance of each line to ground.
Keeping the final differential impedance constant, you can make each track narrower, raising its impedance to ground, and move them closer together, lowering their mutual impedance. This makes it more like a differential pair, less like two separate lines.
On this thin substrate you need to make the traces a lot narrower, so they can be closer together, so the mutual capacitance dominates the ground capacitance. Try 0.25 mm if your tracks can be this narrow, and see how far apart they need to be to get 90 ohms.
Best Answer
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.