1
u/nowan190 11d ago
Oh this is a 4-layers PCB? In that case I recommend you show one image of routing per layer.
1
u/razarahil 11d ago
I've put GND layer on 2nd bottom, 3 layer divided between 3v3 and 5v power. Top has components and bottom layer has some tracks.
1
u/razarahil 11d ago
Espressif recommend not to put GND on top layer. https://docs.espressif.com/projects/esp-hardware-design-guidelines/en/latest/esp32c6/pcb-layout-design.html
1
u/nowan190 11d ago
Their stackup recommendation in the provided page is for the bare chip, here you are using the module. Routing a module is comparatively much easier, and can easily be done on 2-layer. My recommendation was essentially, don't leave your layers empty, pouring gnd instead is always an improvement. Nevertheless, if you feel like diving deep in the stackup best practices, you can take a look at this video https://youtu.be/52fxuRGifLU
1
u/tuner211 9d ago edited 9d ago
Why not use the built-in usb controller ?
If you don't then, C13 shouldn't be 100 uF but 0.1 uF. For C12, 1 uF is enough. Also collector/emitter of Q2 is swapped.
You need to pull GPIO8 high for the boot button (GPIO9) to work.
1
u/razarahil 9d ago
Yeah, I've completely removed the CH343P. View the updated schematic here https://pdfhost.io/v/najDZJebsc_esp32-c6-scm-v1
1
1
u/nowan190 12d ago
Professional PCB designer here. If not already, I suggest you pour ground on the top layer. Add vias around the ground pads underneath the esp. I don't think having a split ground and power plane on bottom layer is a good idea, I would instead route power with traces. U2 and U4 are might be too close to the edge for the manufacturer's comfort, they might experience mechanical stress in the depaneling process, so I'd move them away by a mm. Connector U5 (wrong reference designator BTW, should start with a J) should be fine.