Separating ground planes in PCBs
First of all, before answering your questions, let me make some suggestions about the layout. I have seen your previous post and this has been a good attempt, but:

1.- The "Switching Loog" is too large. (Switching loop is Vin, Trafo, Q1 and R8, you call it,"high current loop", maybe it is no quite precise) And moreover, this loop include the control area. This is really EMI problem!! I suggest something like this.

(Think in current loops always!)

Make smaller the switching loop
- Place R8 near from C1. Really near.
- Rotate Q1 90º clockwise
- Place R6 and C6 as close as possible (acap) from Trafo pins.

After that,


Think about the "Gate net", "Sense net" and "pin 15 from controller net", It must be route separatly! The "gate net" is a radiant net and the others ones are sensitive nets. Route them.
Route  Vin and Enable controller nets.
Complete the route of primary


(The controller has not a Decoupling Capacitor ? Are you sure of this?)

2.- A connector for trasformer sounds a problems maker. Could you solder your Custom Transforme in the PCB? It would be better. If you cann't, I you sugggest a 2 row 2 columns conectors. In this way you can gain more space between primary and secondary, and more space between trafo pins.

OK and now. Your questions.

1.- Yes, try to keep separate switching ground from control ground, but connect to the same ground, in your case Bottom layer. For this, try to keep the "switching loop" components together according the placement I suggest.

Connecting R8 to Vin through one track and then one via to GND is not a good idea in your current layout.

2.- Ummm... I would try another layout before consider this question.

3.- I cann't undestand this question. What do you mean?

4.- As a rule, It better If you fill the empty area with hatched copper. It improve the etching process in PCB manufactureing.

5.- As a starting point, fill as much as you can. Do you need consider any electrical isolation between primary and secondary.

Good luck!