Even though you have not said, it is clear from the shambolic routing that you are doing this layout with the autorouter. This is such a simple PCB that you can place the devices where the applications notes advise and then hand route it. You will end up with a much better layout. Also, you should add about 10uF of decoupling electrolytic at the GND and input pins of U3. You have not said but depending on the LED strip, the board may be carrying a current of several hundred mA or maybe more so skinny tracks will not cut it. Make the GND tracks into a Copper Area on the bottom layer, make the Vin tracks as wide as possible and then route the Vin and the tracks to and from R1 at about 1mm to 2mm.

Sorry, my bad: "...and then route the **Vout** tracks and the tracks to and from R1 at about 1mm to 2mm."

Thanks for all the info.   Yes this was autorouted.  I never tried manual routing so far. How does this look for a first manual attempt?  (I didn't add the extra cap over U3 yet)  At the very least from what I've read I should still clean up the traces to not have the 90 degree corners. (Oh and the large empty space top left is so I can fold the power regulator flat against the board) I'm not sure what you mean by the "route ... at about 1mm to 2mm".  Does that mean leave 1mm to 2mm between the track and any other track/component? I'm also not sure if I should try to put as many of the non-ground tracks on the top or whether the bottom is fine. I think in theory the max current for the strip is as high as 3A  (20mA per led * 3 led per pixel * 50 pixels). Not sure how wide the track would have to be for that.  In practice I won't be running things at full brightness so actual current should be significantly lower.

Cleanup attempt: 

"route ... at about 1mm to 2mm" refers to track width not clearance. Add the extra cap across U3 before you do any more layout. You can route all the non-ground tracks on the top. Rotate R1 180 degrees and route the (now) bottom end track round the lower edge of the connector, TB1. If you also rotate C1 and connector U1 by 180 degrees then you can tidy the routing a bit more. Set routing to 45 degree corners in the right hand panel Canvas attributes. If you are going to lay U3 flat then assign a horizontal mount footprint to it and then do Update PCB... You will need a footprint with a mounting hole to hold the regulator down. What about board mounting holes?

BTW, the prefix U is normally applied only for ICs. Connectors are things like P, PLG, S, SKT, CONN, J, JK (for Jack). If you add mounting holes put the symboks in the schematic and then do Update PCB... If you bolt U3 to the PCB, make sure there's either clearance round the hole to not short the tab to ground or use a nylon bolt or a steel one with an insulating bush. Although he probably does not need heat sinking, you could add some Vout top layer copper flood around it and just solder the tab to it. It's such a simple board that if it fails you could just replace the whole thing. You get a minimum of 5 PCBs anyway from JLCPCB.

Rotating TB1 180 degrees might help routing too.

I'd rather not rotate U1; I prefer to have GND at the right hand side for screw terminals.  (I suppose I could/should look up how to add text to the silk screen and just add +5V and GND markers, but simple convention has worked for me so far) Any hints on how to pick the correct horizontal footprint?  I went with TO-220-3_HORIZONTAL but I'm not convinced the dimensions are actually right. Guess I should just measure and verify ? Haven't actually mounted any of my boards but yes I might as well add mounting holes. As for the prefixes, those were all auto-assigned. I'll try and update them manually to be more appropriate. Rotating TB1 would unfortunately cause the ESP-01 to hang off the board.  Unless I move TB1 to the top after rotating it, and either move or rotate U3 as well. I'll see if I can play around with it a bit. Once again thanks for the comments and advice. I've learned more from this short thread than from days of googling and experimenting.

@desmej, You're welcome. :)

"I went with TO-220-3_HORIZONTAL but I'm not convinced the dimensions are actually right. Guess I should just measure and verify ?" You should always check every symbol and footprint against the manufacturer's datasheet, irrespective of which library it comes from but especially if it is User Contributed. That said here is one I made earlier and have verified in a project of mine: STP62NS04Z\_HORIZ\_HAND\_SOLDER  STP62NS04Z_HORIZ is the same but has no hand tab soldering hole, just the bolt hole. I built it for this device: [https://uk.rs-online.com/web/p/mosfets/7610152/](https://uk.rs-online.com/web/p/mosfets/7610152/)<br> <br> so you will need to re-map the pins to your regulator.

One more question\, about the extra decoupling cap\.   You said to add it between the input and GND pins of the regulator\.   That would really put it across the same lines as the C1 cap\.  Does the physical location matter that much that C1 isn't close enough to also act as a decoupling cap for U3 ?     Or was that a typo and it should be between the \_output\_ of U3 and GND ?

Doh! Not sure if that was Autocorrupt or senility... Yes, that should be output and GND of U3. Check the recommendations in the device datasheet. If the track to the input pin of U3 is left thin then adding about 100nf from U3 input pin to GND might be wise. Otherwise, just make the Vin track a copper area so that the connector pin, C1 and U3 are all connected by maximum copper, which light necessitate rotating U2 as shown in the above screenshots to simplify that task. Remember that components have to be placed according to electrical requirements first and mechanical requirements second. It's no good having stuff fit neatly in the box if it doesn't actually work. :)

Ok attempt number not-sure-how-much.  Bottom of board is a ground plane, top of board is 5V plane. Added the extra cap and mounting holes, and replaced the ESP header with an actual ESP  (even though I'll still be putting on an actual header; but at least this way it shows how it will look when plugged in), and moved things around a bit. 

The antenna on the ESP must not be screened by PCB copper. Please study recommended placements in the the apps notes for the ESP: [https://www\.espressif\.com/sites/default/files/documentation/esp8266\_hardware\_design\_guidelines\_en\.pdf](https://www.espressif.com/sites/default/files/documentation/esp8266_hardware_design_guidelines_en.pdf) from here: [https://www.espressif.com/en/products/socs/esp8266](https://www.espressif.com/en/products/socs/esp8266)

Yikes that's a lot of required clearance. Guess hanging it off the board might be the easiest way to go.  And looks like the main takeaway from this is starting to be "find and read the specs for any component you use".

Absolutely! And try to find the datasheet and apps notes from the original manufacturer not the stuff copied onto distributors and other 3rd party sites as these are often out of date, incomplete or superceded. :)

Two sanity checks: 1. Is there room under U2 for R1? 2. Is there a risk that the mounting bolts, nuts and washers may end up shorting the GND and 5V copper areas if the solder mask is damaged? Similar comments apply about the clearances around the holes or the use of nylon bolts as given for U3 above.

To answer your much earlier question about track width vs. current: For calculations of trace width vs. current vs. temperature rise, see this topic: [https://easyeda.com/forum/topic/PCB-high-current-thermal-design-562f7a69a7ad41a38b18ea150d6703ed](https://easyeda.com/forum/topic/PCB-high-current-thermal-design-562f7a69a7ad41a38b18ea150d6703ed)

"Similar comments apply about the clearances around the holes or the use of nylon bolts as given for U3 above." That's the voltage regulator that is now shown as U1.