Having the schematic would greatly increase the range of advice that could be given depending on how full of a review someone was willing to conduct. A review based on gerbers alone for instance would never have revealed an addressing conflict.
It would be a good idea to post the schematic as an image or pdf however, to save everyone from having to load your project into Kicad.
You have no idea how common that is. I'm willing to bet that when you wired up your breadboard you used something close to 22 AWG wire. That has a cross sectional area of 0.3mm2 compared to your 10 mil PCB tracks which have an area of 0.009mm2. You also probably wired your power and ground with more of a star topology. So all of your ICs would have had a relatively low impedance connection to the power supply while the impedance on your PCB will be significantly higher. The same circuit on a PCB might not work at all or if it does it might not be very reliable. Your processor might reset every few minutes or hours. It might work fine until you change a piece of code, then you spend hours/days debugging your code when it is the hardware that is at fault. It might even be temperature dependent.
You can google for more information on decoupling capacitors, you can also read this post: https://forum.kicad.info/t/ground-plane-filling-every-space-orphans-solved/5146/22
Forget everything you have ever heard about right angles on a PCB. When people talk about "right angles" they are usually referring to right angle corners, ie "L" shaped corners. While there are technical reasons to avoid "L" shaped corners they don't apply to most layouts. Most people avoid them because they heard somewhere that they were bad or for aesthetic reasons. If you don't like the look of right angle corners then miter them with a short 45 degree segment. But the same does not apply to "T" branches. If you are doing a layout where you need to avoid "T" branches for impedance reasons then branching at an angle is not going to help.
As for the vias, they take up more space than a track so it is always a good idea to avoid them. You also don't want to be hopping from one layer to another any more than necessary.
If you look at your R3 & R2 you see a via next to the resistors through-hole pad. Obviously there is no need for the via. But even the track that connects to R1 switches layers when there is no need. There are several other such tracks. And if you clean some of them up your planes will become a little less segmented.
For a start examine the ground connections for J6, SW1 and J9.