Looking for feedback on switching power supply board design
Your second layout looks good, nice job!
For radiated noise the priority is minimizing your hot loop: Current out of Cin to Pin1, out Pin 2 to diode, out diode to ground, back to Cin. I'd probably widen the line from pin 2 to the diode a lot. As was mentioned in a comment, moving to SMT parts will improve ESL and ESR to some degree. You have everything well routed on the top layer so the vias don't really matter, it's just that SMT components are better. What you've got looks good but we're always paranoid and do everything we can, right?
This is more a design than layout comment, but... A priority for output voltage ripple is Cout value and ESR. Try to get close to the 30mOhm limit of that part (per the datasheet) for the big caps, combined. I'd consider adding a high frequency capacitor on the output. The switcher is only at ~50kHz but the rising/falling edges of the switching waveforms are very fast and will be well into the MHz or 10's of MHz of content. So, put room for one or two 1uF SMT caps on the output.
I don't think it would actually matter but I'd pull the ground plane closer to pin 3 to minimize that trace length/inductance.
I prefer larger annular rings for L1 and U1 thru-holes. For rework of U1 for example you might heat and reheat the leads several times trying to get all the solder out. It's easy to delaminate the annular rings when doing that. Same for L1. For hand soldering, I make those annular rings pretty huge.
Another personal preference is that I'd add a pair of 0.1&quot; header pin vias on the board for Vin, gnd, and Vout. I'd solder a loop of wire on those so I could easily clip multiple test leads on them (ez hooks and o'scope, alligator clips, etc.). A single pin can be annoying with multiple leads connected, for me, anyway.
Again, nice work it's looking quite good. If you fabbed it as is I think you'd be quite happy.