4-layers seems overkill for a project like that (2-layer should be sufficient). I've always used the bottom layer (2-layer PCB) as the GROUND, and then do a copper-fill for the entire layer.  All the other traces are usually simply on the top layer (with a few extra on the bottom).

England Rasmussen, Please read (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) and then find **Sharing** in the Tutorial (1) in (2) in the above link. You will also find out how to create copper areas in the Tutorial. Many of your traces are far too narrow and the loop areas enclosed by them too large. I suggest that you pay close attention to the layout guidelines in the datasheet  for your chose amps converter chip. Open and study this project for a helpful example of a buck converter in EasyEDA: [https://easyeda\.com/example/Automotive\_12V\_to\_USB\_5V\_2A\_output\_power\_adapter\_\-L1xrlfxrJ](https://easyeda.com/example/Automotive_12V_to_USB_5V_2A_output_power_adapter_-L1xrlfxrJ)

Ok thanks bwinter, your answer was very helpful. I realized once you make the ground copper fill that the tracing becomes a lot more straight forward. Andyfierman, I was not able to find information of what the trace size should be for 3A supply. Is there a resource you can direct me to? Thanks guys :)

@rasmussenengland, It's not just your trace widths it's having long runs between components carrying fast edged currents. You need to look at the layout guidelines: Sections 8.2.2., 8.2.3 and 10 in: [https://www.ti.com/lit/ds/symlink/lm2678.pdf?ts=1603870252694&ref_url=https%3A%2F%2Fwww.ti.com%2Fproduct%2FLM2678](https://www.ti.com/lit/ds/symlink/lm2678.pdf?ts=1603870252694&ref_url=https%253A%252F%252Fwww.ti.com%252Fproduct%252FLM2678) and: [https://www.ti.com/lit/pdf/snva021](https://www.ti.com/lit/pdf/snva021) [https://www.ti.com/lit/pdf/snva054](https://www.ti.com/lit/pdf/snva054) For trace widths vs. copper thickness, current and temperature rise, there are a number of online calculators available, based on the graphs that @cjohnson kindly uploaded in his preply to this post: [https://easyeda.com/forum/topic/PCB-high-current-thermal-design-562f7a69a7ad41a38b18ea150d6703ed](https://easyeda.com/forum/topic/PCB-high-current-thermal-design-562f7a69a7ad41a38b18ea150d6703ed). For example: [https://www.7pcb.com/trace-width-calculator.php](https://www.7pcb.com/trace-width-calculator.php) [https://www.4pcb.com/trace-width-calculator.html](https://www.4pcb.com/trace-width-calculator.html) [https://www.desmith.net/NMdS/Electronics/TraceWidth.html](https://www.desmith.net/NMdS/Electronics/TraceWidth.html) [https://www.smps.us/pcb-calculator.html](https://www.smps.us/pcb-calculator.html)

 Ahh, I see :) thank you for the information andyfierman. I moved my components around to make the runs shorter, added a copper fill layer for the ground, and thickened the track according to an online calculator. Do you see any other glaring issues that I could cover? Are tracks (w) the same thing as a copper trace connection between two points?

"Are tracks (w) the same thing as a copper trace connection between two points?" Yes. Tracks a.k.a. traces. Without sight of your project to check on component values and a spec to describe input and output voltage and current requirements I am guessing but I think your output caps look very skinny compared to the size of L1 so I suspect they will not have a sufficient ripple current rating (they will overheat and at best dry out and then explode or at worst, just explode). Again, read the datasheet: do the maths. Also, rotate C1 & C2 180 degrees to reduce the loop area around C1, C2 L1 and D2.

Thanks andyfierman, your help has been very valuable. I actually tested the design on a breadboard according to the datasheet and did my due diligence on the component selection. :) I already ordered the pcb without the cap rotation lol. I think the design should work fine now that I figured out all the earlier mentioned difficulties. Ill update the thread if I run into any issues further down the line. Again, THANKS!

Thanks, glad it was helpful. BTW: I don't think you'll find too many sources recommending breadboarding switch mode supplies...

Hello! There might be a problem with the electrolytic capacitors. The power traces are creeping way too near the negative pins. Making the power traces a bit thinner might solve the issue. Regards, Markus Virtanen HW / Electronics Designer

The input and output voltages haven't been stated but it can't be more than 40V for that smps chip. A quick check on a creepage and clearance online calculator will sort that out: [https://www.smps.us/pcbtracespacing.html](https://www.smps.us/pcbtracespacing.html)