How to correctly connect low current analog ground plane with high current analog ground plane on PCB?
The question that needs to be asked is: &quot;Do I need separate planes?&quot;
The answer is usually &quot;No&quot;
Here is why:
By separating the grounds, there is only a small piece of copper in between the two planes. This copper has inductance and resistance, so what is done in this design is like putting a small inductor and resistor between the two planes.
The resistor made from the trace will be about 1mΩ with maybe 1nH of inductance, which will make a filter on the ground for the left half of the board. Any current moving from the left hand side of the board will flow through this point and create a small voltage through the resistor/inductor trace.

The biggest problem will be IC2 (blue) which the signals connected to it are referenced to the right half of the board and it's ground is referenced to the left half of the board so any difference in voltages on the grounds, which could be in the mV's depending on the current.
Another problem is the entire ground plane forms a nice dipole antenna, which could also create EMI problems or ring at high frequencies.
So unless there is a good reason, don't split the planes and combine them and let everything be the same potential. The best way to deal with return currents is with board layouts that rout the currents to the right paths (currents take the path of least impedance (resistance) or the orange lines. And it looks like the current's won't cross anything important (if they do a chip that is ground referenced might see the currents, V=IR and ground planes have resistance).
If you want to eliminate a ground loop (like if the connectors are connected to other devices) then isolation is the best (like optocouplers or digital isolators)