I agree that now enough effort has been put into the 2-layer routing that going back would be a waste. But these days my preference for all but the simplest boards is to go 4-layer (with inner layers dedicated to ground). It makes the routing so much faster, and generally the end result will be better.
For prototypes it’s a no-brainer, at JLC the cost is $8 instead of $2 and I’ll be spending $7 on stencil and $15 on shipping anyway.
I found a few other places I could do better… Tried reducing the amount of vertical traces on the back side. Added a few more via’s.
Now for some work on the schematic…
It’s looking nearly finished…
I still see the thermal reliefs around the mounting pads (mentioned earlier by eelik) you can make solid connections by hovering over the holes and press e for edit.
There are a few long horizontal tracks near the bottom, and a row of connectors on the bottom side of the board. How are the currents going to and from those connectors?
I think I still see a ratsnest line at the double row connector at the right top side. Make sure you do a DRC check when you’re finished.
I don’t know your goal with the zone in the bottom right, but stuff like this could cause problems: 
Who have you down-selected to fabricate the card?
Have you cross-checked your card constraints
That TO220 could be replaced by a SOT223. The size of the tracks from it implies a low current such that a decent SOT223 will do
Those buck could be wired in parallel from the 24 rather than cascade to help with efficiency any maybe routing
Found that… Yeah, I like that idea. Although, the board will be attached to a raspberry pi with nylon standoffs and housed in a plastic box, so I’m not sure how important those mounting holes will be for grounding, although one never knows…
Which connectors are you speaking of?
I addressed that. That pin is powered by the raspberry pi, so it’s really not an issue. However, just to make DRC I marked it unconnected on the schematic.
That is supposed to be an isolated area for a device that requires digitally isolated power.
Either JCLPCB or PCBWAY. Although I’m not entirely clear on how PBCWAY prices assembly. Still thinking about it. I had an early version of this done by JCLPCB and was happy with the results.
I thought about that, but decided to stick with the TO220. I didn’t find a SOT223 that had the same characteristics as this particular piece. I intend to bend the pins over and lay it flat against the board. The board is going to be mounted in a plastic box and then the box will be mounted on the side of my aquarium stand, so it’s in a very low vibration area. I’m not concerned with it being damaged.
I actually hadn’t thought about that.
Not a huge help in routing, creates another large trace on the backside. But I can see where it would help with efficiency for sure.
You should have your isolator straddling the zone cut then. As it is, you’re creating an enormous loop for the return current of those signals.
Not looked carefully over everything, but night and day improvement from your first version.
Any reason why the bottom-right pad is not associated with a net while the other 5 are GND?
That bottom right pad is in some isolated area. It may be a good idea to increase the clearance around that pad a bit just to make sure a screw can not get connected to the zone.
Another thing you can do is highlight your tracks one by one to check for “weird loops” in their routing.
Ahh yes good point. Then yes pull back the separation
Not sure the best way to do that. Also, I’ll be using nylon hardware on this, so I don’t think it’s going to be much of an issue.
What do you mean by “weird loops” ?
Try Inspect -> List Nets -> choose any given net and it will highlight that set of traces alone, which helps find any odd quirks. Sometimes fixing / re-laying one trace will create room to optimize others.
I would add at least one 10nF cap across the gap between the ground planes.
This has been an education for me. thanks to all the contributors.
Me too… Regardless of how I may have come across, I did learn quite a bit from this.
