I have designed a PCB in Eagle. I have doubt regarding creating the ground planes. I have created a ground plane on the top layer only

PCB Design

But I even have connections in the bottom layer too which are nothing but the ground connections to the MCU.

  1. Do I have to make another ground plane in the bottom layer for sure or can I order my PCB right away?

  2. If I have to create ground on bottom layer, too: Do I have to connect the top and bottom layer ground planes using VIAs?

Antenna Datasheet

Datasheet of the MCU used

  • 1
    \$\begingroup\$ You can't order the PCB, you have DRC/ERC errors on some of the via's. \$\endgroup\$
    – Ron Beyer
    Commented Jan 8, 2020 at 18:54
  • 1
    \$\begingroup\$ Put one on the bottom as well, add some Vias and Name them Gnd to connect the two layers. Double sided boards are pretty much the standard. You have a component labelled "ANT" is that for antenna? Check its datasheet, you probably Don't want Gnd plane under that one. If it's pads for and offboard antenna, then Gnd plane is okay. \$\endgroup\$
    – CrossRoads
    Commented Jan 8, 2020 at 19:14
  • \$\begingroup\$ @CrossRoads see my answer... \$\endgroup\$ Commented Jan 8, 2020 at 19:16
  • \$\begingroup\$ I see Gnd Traces now too, vs a Gnd plane. Not good. Draw a Polygon on the bottom layer around the whole board, Name it Gnd. Hit Rats Nest to implement it. I can't edit older comment to take out the antenna part. \$\endgroup\$
    – CrossRoads
    Commented Jan 8, 2020 at 19:19
  • \$\begingroup\$ Much better now! \$\endgroup\$ Commented Jan 10, 2020 at 11:28

1 Answer 1


your questions

Do I have to make another ground plane in the bottom layer for sure or Can I order my PCB right away??

Come on, making a ground plane really isn't hard.

Generally, I'd go as far as saying that the bottom ground plane is more important than the top ground plane: It allows for return currents to flow exactly below the traces on the top plane.

So, yeah, add a bottom plane. While you're at it, a single via in a large top plane really isn't great for impedance. In very high frequency applications, it actually has the potential for making your top plane a patch antenna – which is the opposite of what you wanted.

If I have to create ground on bottom layer too Do I have to connect the top and bottom layer ground planes using VIA's?


other things

  1. There's a component labeled "ANT" on your PCB. If that's an antenna, it probably requires a ground plane. Read that antenna's datasheet carefully!
  2. if it's an antenna, the trace below it and right next to the trace leading there are probably very bad ideas and will couple a lot of RF energy.
  3. if it's an antenna, then the connection between the large IC and that needs to be a transmission line of specific impedance. That also requires a ground plane. Like this layout looks now, chances are you're coupling most of your RF energy into the surrounding traces instead of between antenna and IC. If this is your first RF circuit, follow the examples set in the datasheet and application notes of the IC manufacturers. RF is hard, you might want to read a book on basics of transmission line theory, at the very least.
  4. You put a "ring" around your IC, probably something like VCC for that IC. Don't do that. That literally makes that trace a secondary winding in a transformer that picks up some RF or inductive coupling from power lines.
  5. If it's VCC: decoupling capacitors belong close to every VCC pad. Not only close to a single one.
  6. why exactly are you making a small loop next to the 10k resistor instead of simply connecting the neigboring pads?
  • \$\begingroup\$ Comments are not for extended discussion; this conversation has been moved to chat. Any conclusions reached should be edited back into the question and/or any answer(s). \$\endgroup\$
    – Dave Tweed
    Commented Jan 9, 2020 at 21:49

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.