I'd go for number 1 because there is no chance that spikes caused by digital chips on the "red" rail can enter the analoge part of the red. BUT BUT BUT...

You need to explain what external analogue inputs there are and how they retain isolation from ANY ground local or otherwise. This could be a killer without decent differential inputs or some other form of isolation.

You also need to explain what may or may not be grounded on the circuit board and the capacitance across the transformer that creates the basic DC supply. If battery powered then no probs.

Some basic stuff

Do NOT split the ground plane

If you've read the comments you'll understand that none of the engineers here (myself strongly included) think that you should split the ground plane. In your application it will hurt more than help (most most most likely). The way to intuit about planes is to recall that the thing that matters the most is the circuits' loop area.

The loop area is the enclosed region between the outbound and return circuit traces in 3D space. When you split the ground plane you will create some paths that look like this:

The outbound path goes direct, but the return has to take a much longer (and distant) route resulting in a large loop area. This makes it radiate (and receive radiation) much more efficiently (not desired).

The other issue in play here is that current follows the path of least impedance (NOT resistance). The high frequency elements of the current will follow (as best as possible) the outbound path, but the low frequency elements will follow the shortest path. This variation means that even if the loop area is low for some band of the energy, it may not be for others:

A solid ground plane, with good component placement, will give you the best of both worlds.

Increase your decoupling at the digital IC's power pins

This is the best layout:

...and these parts should be placed immediately adjacent to the Digital IC's power pins. Ideally:

multiple vias to power plane/track --> Capacitor's positive pour area --> IC pin.

Make the board thinner

Remember the all-important loop-area? It bites you again with a 2-layer board. In a 2-layer board, the full-thickness of the PCB is the separation between outbound and return current paths. If you make the board 1/2 the thickness, you will 1/2 the loop-area without changing your layout at all! With a 4-layer board at standard 1/2 thickness (0.8mm) the path separation will be around 0.26mm (e.g. 1/3 of a 2-layer board of the same overall thickness). That means a 4-layer board would be 3 times better at reducing cross-talk and unintended radiation (first order approx).

Maybe not possible?

Look, you might just be asking too much...

• 24-bit ADC is extremely sensitive
• 1GHz switching in a digital IC is very fast
• 2-layer board implies broken planes and wide plane-to-plane separation