Potential Difference in the Ground plane
My colleague told me that there will be potential difference between
PGND in bottom layer and AGND of analog section and it is not good for
the design but my understanding is that if I have intact ground plane
then it will not be any potential difference.

There will be a potential difference, if the ground plane was made from a superconductor, then there would be negligible potential difference. All materials have resistance.
Ground planes can be imagined like a grid of resistors:

Source: https://www.mathpages.com/home/kmath668/kmath668.htm
This means that any current from point to point on the ground plane will generate a voltage, but it will be very small. 1oz copper has a resistance value of 0.5mΩ/square inch. The value of the voltage that the ground will change still follows V=I*R but the problem is with the resistor &quot;grid&quot; (which actually is continuous) currents are 2 dimensional. In the image below lets suppose the point Vb is a higher voltage than Va, current will flow in all resistors, but higher in the ones between Vb and Va. Now imagine the resistors are a continuous piece of 1oz copper, and the points are vias.

Source: https://rosettacode.org/wiki/Resistor_mesh (modified by me)
The amount of voltage that will be generated by currents can be estimated, with 0.5mΩ of resistance per square inch, 1mA of current would generate ~5uV of voltage on the ground plane.
In analog designs, a designer needs to first consider if ground plane effects will really be a problem (if your design is on the uV or nV level, then it will).
If it does, then currents will need to be reduced with isolation OR by proper component placement. Currents will always follow the lowest impedance (or for DC lowest resistance) path back to their source. If you have a load that sends a lot of current through the ground plane, it can cause sensitive analog electronics to see the ground change, which contributes to noise and error in the signal.
So your diagram actually looks like this:

And Rg could have other currents flowing through it from other components. From the diagrams above, I cannot tell exactly what these would be, it requires a schematic and usually a good look at the CAD and a knowledge of all the currents and the locations of these on the PCB.