How do I separate ground planes on a PCB with two different voltages?
Simple answer is you don't split planes unless you know what you are doing and why you are doing it.
Separate the ground planes and route signals over the the gap in a split ground planes at your own peril.

The lowest inductance path for return currents is on the ground plane directly under the signal trace. This forms the smallest possible 3D loop.
But the return current from such traces cannot cross the gap in the split plane so will flow around the gap instead making a big fat loop.

You do not want to split a plane without justification because you then can only route traces over the bridge between split planes or else you end up with the aforementioned big fat loop.

Instead, what you do is just use a single unsplit ground plane but partition components to different areas on the board so ground currents of the noisy parts do not flow through the ground plane under the sensitive parts.



The only cases I know where you might split the plane is you need really, really low noise but can't partition sensitive section of the PCB far away enough.
Current flowing on a plane kind of spills out and smears to the sides of the linear path it is taking. Split plane can stop the spillage from leaking onto areas of the plane that are under other components because you cannot space them far enough in your partitioning with a single unsplit plane. But it's still contentious whether this is actually needed.

Images taken from:
http://www.hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf