Two layer FR4 PCB: should you place GND pour on signal layer?
Most of the work is done at component choice and especially placement stage. If layout gives you headache, it's most likely a placement problem.

#1 so many thermal vias for such a tiny copper pour, why not get a regulator that has the tab at GND to use whole GND plane as heat sink?
#2 This power trace shound be on toplayer, use vias for signal traces to pass under the power trace instead. That will end up needing a lot less vias than the ground stitching you did.
#3 No need to put so many vias on that capacitor's ground pin, if there's only a tiny one on its power pin... Impedance of both pins is in series.
#4 Shaking the placement a bit should remove lots of vias here.
#5 Same, if you wiggle the traces around, a lot of vias can be removed.
#6 Note the trace in the power pin of the cap is in series with its impedance, so if you want good &quot;HF&quot; (quotes because electrolytic) frequency performance for your ripple filtering, that's not how it's done, instead you route the power trace through the cap pad. You could space the connectors on the top and put the caps between them. More spacing will also make it easier to grab the connectors with fingers. Btw always print the PCB on paper and stick the big parts in it to see if they fit, sometimes you get surprises.
I notice big traces (implying big currents) ending in tiny vias. Did you check the current capacity of your vias?
Several things look like MOSFETs, perhaps they need copper pours on the tab as heat sink? Note a copper pour on toplayer will sink some heat through the board and then into the ground plane on bottom layer, so you get both sides cooling. It's not very effective, because FR4 has low thermal conductivity, but copper is free, so why not.