Need feedback on my new circuit design
It's hard to find useful layout documentation to your ESP8266-12E; but I bet the antenna mustn't be placed above signals, and it's likely it shouldn't be placed above any copper at all. Espressif themselves have reference designs where the antenna should be sticking out from the rest of the board: 
It's a good idea to route signals on the top layer, sure, but not because your board is single-layer: every board house I've met will give you the same price for single- and two-sided boards. You want the bottom side to be (almost completely) reserved for a ground plane. You want your decoupling capacitors to be able to take a short current return path – otherwise, they're useless, or worse, they even distribute noise into other systems.
I don't know your relay type, but I think something is very wrong in your component footprint: in all sensible relay designs, the three &quot;high voltage&quot; contacts are on one side, and the lower-voltage coil is on the opposite. So, verify with your relay datasheet how your footprint looks like. That pretty much changes the largest part of your relay board layout, so re-do that (from scratch).

(did I mention datasheets? Save documentation to all your parts with your project; if a part has no datasheet, go to a reputable distributor like farnell or digikey and buy a part with a datasheet instead.)


I don't know your 220 V AC -&gt; 5 V DC supply, but usually, if there is a rectangular box, you can't put a resistor in there – don't R10, R11 collide with the supply?
as your layout software indicates, you've basically split your top-layer ground plane in half on your relay board with the long horizontally running 5V rail. That won't do well, but doesn't matter because I guess you'll be re-doing that layout with the correct relay pinout, anyway.
generally: layout the relay board such that all high voltage is on one side, and that there is absolutely no board copper crossing from the high-voltage side to the low-voltage side. Again, your relay footprints are almost certainly wrong, and that's what makes this harder. Google &quot;PCB Clearance 220V&quot;. You never want your high-voltage circuitry to be close to your low-voltage one, and your design doesn't allow for that separation. That also means &quot;no ground plane under your relay's dangerous side&quot;.
You're missing decoupling caps at the shift register (it's not what we'd normally call an &quot;IO expander&quot;, it's a just a shift register). Adding one close to each relay would also make the whole system more robust.
Your relay board (the other one, too, but here it's a real show-stopper) needs mounting opportunities: some holes to put a screw in, or free edges to slide it into some guide or something. Mounting is necessary, because the bottom of your board will have 220 V contacts sticking out – can't have that flying around, or you will at some point either touch it or have some dirt cause a short and then a fire.
Print out your design in &quot;real&quot; size before ordering it. This is probably smaller than you think it is (always happens to me, still, after years), and since boards are cheap, making things larger is always a good idea