Have you gone through the checklists, (4), (5) and (6) in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) ?

@andyfierman Thanks, I have gone through it thoroughly beforehand. I'm mainly asking because i'm about to order it and as many people before me, am quite anxious in case I missed anything.

Your use of netnames to declutter the schematic is OK you've gone too far with and the layout makes the connectivity very hard to follow. You could have used Busses and a few more wires to make it all much more readable for anyone who is trying to help. Recommend you use maximum copper for ground, 3.3V and VCC supplies. Widen the traces and use Copper Areas where possible. "Quick recap of the schematic:" It's not a recap. Nobody but you has seen this before or knows how this is supposed to work. A more detailed How it Works type of description would be more helpful. A Design Requirement Specification would be even better. :)

@andyfierman thanks for the input! As for the 3v3 and the 5v supply i will make them larger although I calculated that it should be more than enough already, but since the area is available why not Sorry for the recap, I tried to keep it's description as brief as possible, a more detailed but still very brief description follows: The main requirements were to design an expandable matrix, meaning that a single board will be able to control a 4x4 matrix with the possibility to expand it by adding more boards. This design language was used to keep the cost down since this is just a proof of concept for a larger university project. The 4x4 matrix consists of IR receivers and RGB leds, having a global bus for the IR signal and having the Darlington sinks provide ground to each and every cell individually, this was so an external power source can be used for the matrix, since it will be physically placed away from the board.  Off board logic converters(fig.1)  were used in order to shift from 3V3 to 5V, the reason they were not implemented in the SMT process itself is because that only one board requires them.Various jumper headers(fig.2) are placed in order to turn on or off the debug LEDS placed in the board as this will mainly be used for testing purposes. Middle array for the matrix, left strip for the Shift register output and the bottom 4 for the shift register input.  In fig.3, the PTH dip16 component is the 4555 decoder which provides and active high signal that feeds the array of transistors. 4 outputs on the X direction and 4 outputs on the Y direction. This is basically the matrix, having the transistors used as AND gates and providing 16 possible outputs. Which as stated before, then feeds the Darlington transistors (fig.2 yellow pen) which turns the active high into a ground connection. 

Also to add to the above: the application is expected to be driven at very low frequencies. so some trace angles, although unconventional should not have any adverse affect.

You now have some copper areas that are floating. This can cause odd effects with crosstalk and EMC so either connect them to ground or supply as required or set **Keep Island** = **No**. Also set **Pad Connection = Spoke** otherwise you will make the board unsolderable because the copper areas will suck the heat away from the pads. Somewhat confusingly, the spokes are also referred to as Heat Shunts: the narrower they are the less heat they shunt away from the pad but the higher their overall impedance. At your operating speeds (and for the most part it's actually edge speeds that matter not clock frequencies), however, that is not an issue. Neither is the shape of any track corners: there are field solver simulations that show that edge corner shape doesn't have a significant effect up until the high microwaves). Add copper areas  on the other side of the PCB for 3V3 and VCC. Particularly when using CMOS devices, it's just as important to have a low impedance path to the supply rails as it is to ground.

@andyfierman Thanks for the input! I have now done widened the VCC and 3V3 tracks to 0.7mm, along with the ground tracks that are connecting the islands. I have also widened their Vias to 0.9mm and 0.45mm drill diameter is this considered "enough"? as I 've read they should be at least the side of the track you're working with.

"I 've read they should be at least the side of the track you're working with." I've not seen any specific recommendations for that but it won't do any harm. Check for spurious tracks creating 45 degree spokes as in this topic: [https://easyeda.com/forum/topic/Cross-probe-and-place-78f0e5019bea46e1b0baf5821c3754ac](https://easyeda.com/forum/topic/Cross-probe-and-place-78f0e5019bea46e1b0baf5821c3754ac) Out of curiosity: is this hand or autorouted?

@andyfierman Sorry, I meant size. i'm rechecking my ground connections to make sure i don't have any 45 degree connections to my PTH bottom layer components. This is hand routed, is the routing not too shoddy or? unfortunately to place the components the way i wanted to place them proved to be quite tricky to route certain areas, as can be clearly seen. I'm planning to order the PCB later today, do I have your thumbs up? :)

"make sure i don't have any 45 degree connections to my PTH bottom layer components." If you have no planes on the bottom layer than it does not matter. It only matters if you have a trace on the same layer as the Copper Area Spokes. I have some rules about when it is appropriate to use an Autorouter: [https://easyeda.com/forum/topic/Auto-Router-Local-and-Cloud-not-creating-all-trakcs-15926363684e4cb9a8233636627839c6](https://easyeda.com/forum/topic/Auto-Router-Local-and-Cloud-not-creating-all-trakcs-15926363684e4cb9a8233636627839c6) You could probably arrive at a better manual routing with that layout but I think what you have looks good to go. * Don't forget to go through all the check lists AND download and check the Gerbers before you submit to manufacture.

Order has been created! thanks for the tips. Went ahead and ordered 2 different versions of this PCB, just in case something's wrong with the SMD version i have a PTH version that is basically a CC of the prototype I've built. Thanks again and stay safe!