Properly Grounding Analog/mixed ICs from DC-DC Converter
(decoupling) capacitors are local batteries from which the high frequent current is drawn. So, on your PCB draw a line from the positive terminal of the capacitor to the IC it feeds (so, Vdd of IC) through the IC to its negative terminal (Vss) back to the capacitor.

To reduce EMI, the length of the drawn loop should be as short as possible and the area enclosed by the drawn loop should be as small as possible. The current flow that draws the most current and/or has the highest frequency components should have the highest priority.

I drew some current loops on your PCB and indicated a so-called starpoint.
As far as i can see, you nicely seperated the boost converter currents (right of the starpoint) from the DAC ICs currents (left of the starpoint), so here, you probably don't have 'bad return paths'.

=> Is the trace "12V from LDO" in the same PCB layer as the ground plane? Then, the return path from the DAC IC's will be very bad. But I assume it is not the case and the trace "12V from LDO" is in the top layer and the purple coloured ground plane in the next layer.



For boost converters (actually, I think all converters) the most important current loop is from the input capacitor to the Boost IC and back. That's why Layout Guidlines always start with "The input capacitor should be placed as close as possible to the input pin for good input voltage filtering."

I made the assumption the input capacitor is located at the yellow arrow.
To reduce the the current loops of the Boost converter I suggest to swap the input capacitor and the capacitor connected to pin 5 of the IC, and extent the ground polygon under the IC to the right, connecting it to the ground terminal of the input capactor.