i have made a small circuit using ESP-12E here is how my circuit looks like:

enter image description here

Here i have kept in mind that wifi connection should be stable, still i am not able to get the stable WiFi connection. Reason is still unknown to me.

  1. I kept the WiFi antena without below ground plane. So it won't create disturbance in WiFi signal.
  2. I kept the capacitor as close as possible to VCC, but its far from ground, not sure how i could make it close to that.
  3. No complex component is near the ESP8266 chip on the board.

Not sure what is making it unstable. Any suggestions how can i improve its stability in this circuit design.

Thank you!

  • \$\begingroup\$ Basically, you need a ground plane. \$\endgroup\$
    – Andy aka
    Commented Feb 17, 2021 at 12:43
  • \$\begingroup\$ @Andyaka where? \$\endgroup\$ Commented Feb 17, 2021 at 12:59
  • \$\begingroup\$ On your circuit board. \$\endgroup\$
    – Andy aka
    Commented Feb 17, 2021 at 13:04
  • 1
    \$\begingroup\$ I think you need to examine what is meant by a ground plane. Your blue copper is nothing like a ground plane. \$\endgroup\$
    – Andy aka
    Commented Feb 17, 2021 at 13:06
  • 1
    \$\begingroup\$ You should always avoid running traces on the ground plane as much as possible. You have essentially a bunch of useless copper islands cut apart by traces, instead of a ground plane. \$\endgroup\$
    – Hearth
    Commented Feb 17, 2021 at 15:38

1 Answer 1


Your signal and power traces have no ground return path beneath. That alone might be the killer here. If in doubt, the easiest way to achieve that is a contiguous ground plane under all traces.

The fact that you didn't put anything beneath your antenna is good, but not sufficient: Your buttons and traces right next to the antenna are as important as the things beneath it.

In fact, Espressif has a design guide and it's not really hard to follow. They even have a visualization where to put the antenna (and hint: where to not put it, and that's within the board outline), and it looks like this (pick one of these positions, not multiple):

antenna placement

If you really need to place things next to your antenna, leave 15mm space around it. That includes PCB substrate.


So in conclusion:

  1. don't put anything next to the antenna. Don't even put PCB material below the antenna (but honestly, PCB below that just loses you a few dB of signal, at most, due to mismatch and material losses; metal next to the antenna can distort your antenna diagram significantly, and/or absorb a majority of energy.).
  2. Don't route signals on top and bottom: your board is not that complex. Leave everything on top, and if you need to "bridge" something, wherever possible, just elegantly route it beneath a connector or passive component
  3. Have a ground plane, on the bottom side.
  4. Have good ground connectivity. So far, your module is connected to ground but through a single via (that's kind of OK), but your decoupling capacitor is reduced in usefulness, because it's "barely" connected to ground (for RF signals), only through a long trace instead of through a via to a large ground conductor (e.g. plane) very close to the capacitor).

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.