There are probably sometimes compelling reasons to separate analog and digital GND, but as I know in most cases one single GND is better for EMC than 2 separated. Read articles I linked.
I think there are no rationale for this.
If you have one you have no such questions.
Any wire going between analog and digital part should have a return path near it. So one solution is all wires crossing the GND border close to each other and GNDs connected under those wires. The other solution is to connect GNDs with small capacitor near each wire crossing the border. Small capacitor gives the return path for high frequency components of signals but left GNDs separate for lover frequencies which were the reason to divide GNDs.
Typical rule in appnotes for A/D and D/A converters is that GNDs should be connected under that IC as one its part should be at digital side and the other at analog.
Separating analog and digital GND planes should not even be considered for <10bit or so ADC’s, and even then, the main key is still managing how currents flow through the GND plane, and that is mostly defined by the signals above the GND plane (above a few kHz) and DC resistance for DC.
Separating GND planes is always bad from an EMC point of view, and should only be considered when you really know what you’re doing. On top of that, leaving dog bones in GND planes on a 4 layer PCB is simply not done.
All that said, it’s mostly a theoretical excersize for this particular PCB because there is hardly anything on it, and it’s quite possible that your IC’s do not even have a particular fast edges.
And I repeat again:
For improvements, the biggest continuous GND you can get is better, and that means also closing the gaps between the pins of the 40p connector. After that comes filtering for all signals that get onto and go off the PCB.
These and more… Filtering is most effective as close to the disturbance source as possible so if you know that here you have a source you should consider filtering just here and not only at going off PCB.
That is why I just power all digital ICs through ferrite bead (I started to do so in previous century when they were expensive, but now it is not a problem). Digital ICs when switching its output they take fast and high current pulses from VCC and I just want that pulses to be not ‘visible’ at other ICs and at PCB power input. Imagine IC driving a differential signal pair going out of PCB. If it get any pulses at its VCC it sends it directly to the output line that just have high state at that moment.
I often route power tracks first. That way at least power is good, and the rest of circuit works better. Then critical or high impedance tracks.
My suggestion is to find out why a part is there. Parts which have some common task, should be close together. Like an IC and its power supply bypass capacitor. Of course you have an 100nF capacitor from power supply to ground at every ic.
The rest is usually not so critical.
