Schematic & Layout Feedback

I am a beginner with PCB design and decided to use KiCad to create a simple circuit involving an ESP32S Node MCU and two L298N IC’s to control four DC motors.

I’d appreciate some feedback before getting the design manufactured & assembled because it is somewhat expensive and takes a reasonable amount of time.

The main components I’ve used are:

  1. ESP32S Node MCU
  2. L298N * 2
  3. LM2596T 5.0V step down regulator

The input voltage will be a 12V LiPo battery rated at about 360mAh

I’m uploading an imgur link because of KiCad forums prevent new users from uploading files

You have a ratsnest line between L1 and U1 and between D10 and D14. Also seemingly several DRC errors and warnings.

Imgur is temporarily over capacity. Please try again later

I pushed you up one level, you should be able to attach an image.

If you could be, at some time, concern about the L298 power dissipation, you layout doesn’t allow a good heatsink installation.

@hildogjr Yes, I don’t have a footprint for that on my layout but I believe the L298N has some heatsink options which can be screwed directly onto the IC without interfering with the pins whatsoever. Something like this

I was planning to just use those. Would that work?

Thanks for pointing out the ratsnest lines, I’ll take a look at those.

The DRC errors and warnings have to do with some footprints I downloaded for the step down regulator. Something about intersecting courtyards. I would assume that i could ignore those since I’m certain the footprint is right and I can procure the components for assembly?

Or is this something I’ll have to fix by recreating the footprints myself?

Thanks, I’ve uploaded a screenshot of the PCB layout

In addition to my post above, the holes of the U2 footprint looks weird, the yellow area of the holes is very slim, which I assume means that the holes might be too large and/or there will not be enough copper there around the holes.

You have no fixing holes for the PCB.

The pins for the ESP look very close to the edge of the PCB (If that is the edge)

I created the footprint U2 myself, so that might be why its weird.

I used a padSizeX of 1.2mm and Hole size X of 1.1mm for the holes. Including a screenshot of the configuration for the hole.

Would you suggest I change it?

The minimum rest ring (anulus) width ( (pad dia - drill dia)/2 ) is around 0,15 to 0,2 mm for most board houses, meaning the pad diameter has to be 0,3-0,4 mm larger than the drill diameter. For heavy leads like with U2 a wider rest ring is advised, something like drill dia + 2-3 mm. Helps with soldering as well.


As @straubm wrote, a rest ring of 0.05 mm is way too thin. I suggest to look at the footprints in the standard library for common values. There main thing you need to look for is that the pins fit into the holes with some tolerance and that the copper ring is big enough for manufacturing and soldering. If the space is tight because the holes need to be big, oval pads are an option.


L298 is seriously obsolete.

It waste’s a lot of heat, that should power the motor instead. Has to be big to be able to dissipate that heat, and it’s also missing the diode’s internally.

Compare it with for example the Allegro A4950.

Okay, I went back to the footprint and reset the pad dimensions to defaults. The footprint looks like below now.

Here is a screen grab of the pad configuration. It has an annulus width of (1.524-0.762) / 2 = 0.381mm, which is well above the tolerance limit of 0.2mm for the board house I plan to allocate this manufacturing to.

Yeah, I’ve read about the heat dissipation issues of the L298N and the voltage drop issues. But, the voltage drop issues seem to be more magnified when driving low voltage motors and since I’m trying to drive 12V motors hopefully it shouldn’t be too bad.
Regarding the heat dissipation, I’ve re-designed to add some heatsinks.

I don’t want to particularly redo the design just to change the motor driver. Maybe in a future iteration.

Yes, but please make sure the pad holes are large enough for your ESP32 pins to fit in. They look quite small compared to the other holes of the board. If the pins are square, remember to use the diagonal and add some tolerance.

From looking at the board I have, it seems like those are standard 0.1 inch pitch headers soldered onto the board. From the images in this link on Pololu’s website, it seems like the diameter of the pin is 0.65mm.

Since the hole dia is 0.762mm which is > 0.65mm, I am assuming that i shouldn’t have any issues.

Let me know if my thinking is wrong.


As you can see by their drawing, the recommended PCB layout has a hole size of 1.02[mm] (which your 0.762 is way under).

These pin headers typically have pins with a square cross section, so the diagonal would be around sqrt(2) = 1.415 times the given side length of 0.65 mm, which is 0.919mm. So your holes are too small.