Routing and ground pours

Go to the Pre-defined Sizes section:

I am going to add 0.6mm, 0.4mm and 0.2mm track widths. For vias, I usually go with vias that have 0.6mm Diameter / 0.3mm Hole and 0.4 Diameter / 0.2mm Hole.

Now after that we have to edit the constraints of the board so that KiCad doesn't throw an error when we try to place them. Go to the Board Setup and then Constraints.

Here we are going to change a couple of settings due to the size of our board. We need to be able to place smaller vias and traces, so change the Minimum via diameter to 0.4mm and the Minimum through hole to 0.2mm. After that's done, click OK and you can start routing!

Starting with the USB-C data lines, these are what's known as a differential pair, so they have to be the same length as they carry a signal that needs to be in sync with the other and the only way for that to happen is if they're the same length. Start connecting them like so:

Then go to Route > Route Differential Pair

and then click on the USB_DP to the far right:

Then route it to the STM32. That's basically the only component that needs differential routing.

Sometimes for VBUS on USB-C or any other component, you might have vias that can't pass through, so I added a 0.3mm track width in the board settings and it works:

If KiCad doesn't let you place a via on a pad for whatever reason, you can edit the clearance in Board Setup > Net Classes. I set it to 0.15, but try not to set it any lower as the minimum for JLCPCB is 0.1mm:

This is how I routed the Battery charger:

See how I used wider traces for power lines and thinner traces for the other pins. I plan on wiring the I2C lines and INT pins connecting to the BMP580 like so:

I connected them to the STM32 through the underside to save space (very useful sometimes). Also, I hid the silkscreen layer so that I can route easier.

Then routed the microSD card:

Go to the right and click on Draw filled zones and click on one corner and a window should pop up:

Here you need to select both layers of copper and select the GND net. Then you need to change the clearance and minimum width to both 0.2mm and also change the Pad connection to Solid or Thermal reliefs. Solid allows the ground plane to connect to the pads better but Thermal reliefs is good if you need to solder/fix the board as the solid ground plane makes it difficult to heat up specific components. For this tutorial I am going to use Solid but feel free to use Thermal reliefs if you want to be able to solder it later. Press OK and start creating the zone like so:

You want it to look something like this:

Then press b on your keyboard and it should fill the zone automatically (Ctrl-b to clear them).

Now you need to check if there are any holes that don't have any ground plane and add a stitching via (via that connects ground/power planes to cover everything) like so:

You also might see a ratline connecting a piece of the ground plane. This usually means that you need a stitching via in that area.

As you can see, the ground plane connecting to Pin 18 isn't connected to the rest of the ground plane, so we need to add a stitching via there like so:

After connecting everything we are going to run Check DRC which basically checks the design rules and makes sure our board is ready for production.

Then click on Run DRC:

Unselect the warnings and look at the errors. If there are any errors about unconnected pads then you should probably go back and make sure that everything is connected. There are some errors but those are from the parts that we imported like the USB-C and microSD card that KiCad is complaining about the holes:

Those errors are safe to ignore but any others you should probably fix.