I like the big fat blue captions. Those immediately identify schematic sections.
Those dotted lines around the sections however are a bad idea. They mostly make the schematic more crowded. They do nothing that a bit of whitespace does not do better. They also cost an amazing amount of time during maintenance on your schematic. How many times have you changed or redrawn those rectangles?
R1 is usually not to limit the gate current from the driver IC, but to make the mosfet switch a tad slower to take the edges of the EMC, but not too slow, as this would increase power dissipation. It’s value is also non critical, so why use a resistor that is not from the E12 range?
The PCB layout looks quite good. Some small remarks:
I would rotate C1 and C2 180 degrees, this would bring all the via’s to GND closer together and reduces “loop area”.
I don’t know if the extra rows of via’s do something useful. If anything, putting some via’s closer to the IC may be (very marginally) more useful. Put them in “corners” of the top GND plane to stitch them to the bottom.
You’ve made the zones bigger then the PCB outline, which will clip the zones by the PCB outline, but you’ve put the zone boundaries on top of each other. I usually draw them in some weird parallelogram or pentagon shape, and make sure the edges of the zones themselves do not overlap. This makes an individual zone easier to select unambiguously.
One thing I’m missing is the routing of the motor power. When PWM’ming motors (or other high current loads) you need some big filter capacitors, and you also want to decrease the loop area. Twisting the wires keeps them close toether, and the twists also further reduce EMI.
I like to add some separate GND connector or test pin to each of my PCB’s. It’s specifically meant to clip the GND lead of my oscilloscope to.
The GND on this PCB is quite good, but when you divide a project over multiple PCB’s, you introduce GND and other problems. Wheere is the PWM input on J2 coming from? Running a TTL (or uC output) through long (>150mm) wiring is not ideal.
Another important thing to consider is what happens if the power GND lead gets disconnected accidentally. It’s easy to burn up the signal GND wire with a high current, and this is a fire hazard.
It’s just a personal preference, but I prefer to wire connectors similarly to the schematic. That is Power in on the “north” side, and GND on the “south” side.
If this PCB is for testing purposes, then consider adding a LED (+ resistor) to the PWM. This gives visual feedback during testing, and in production you do not have to place those parts.