I'm working on a PCB and want to incorporate a 2.4GHz PCB antenna but am a bit confused on how to handle the ground plane(s). This is a 4-layer PCB with Signals (and ground pour) on the top layer, ground on layers 2 and 3 and power on layer 4 (bottom).

I'm new to the antenna part and have read some conflicting information. Some say to remove ground from "under" the antenna (but not sure what under means - just that layer or all layers). I've also read that a meander-style antenna need a reference ground plane, which I assumed means on layer 2.

So putting this out to the community hoping someone with more experience can help me understand how to hand grounds.

Here is a picture of the PCB - it's just a remote control that will transmit BLE data. Assume I have the 50-ohm impedance matched correctly, how should I hand ground? Remove from all four layers or include it on layer2.

I've tried both and including it on layer 2 appears to be a disaster. But, not including it at all seems to work but I'm not getting great range (I quickly hit -80dBm or higher at 15 feet or less).

For reference, the design is following information I found at https://www.st.com/resource/en/application_note/dm00470410-low-cost-pcb-antenna-for-24ghz-radio-meander-design-for-stm32wb-series-stmicroelectronics.pdf

PCB with Antenna

  • \$\begingroup\$ look at figure 3 \$\endgroup\$
    – jsotola
    Commented Mar 5 at 2:41
  • \$\begingroup\$ @jsotola thanks for the reply. I looked at that diagram at least a dozen times but I'm not sure that it gives me the answer. It mentions a top solder mask and trace, the core and bottom solder mask but nothing about ground. Or is that the point, it's what it leaves out? As in, it doesn't mention ground so the implication is that it shouldn't be there? \$\endgroup\$
    – Nollstead
    Commented Mar 5 at 3:03
  • \$\begingroup\$ I'll mention that I saw an Altium Live 2019 presentation at youtube.com/watch?v=ewXNC971Vfc where at the end (at 47:00) the speaker talks about this exact thing and mentions that on a 4-layer board layer 1 is signal, layer 2 is gnd and covers the entire board. So that seems to contradict the "no ground underneath the antenna". Hence why I say that I'm getting mixed results when I search this. \$\endgroup\$
    – Nollstead
    Commented Mar 5 at 3:12
  • \$\begingroup\$ Please clarify your specific problem or provide additional details to highlight exactly what you need. As it's currently written, it's hard to tell exactly what you're asking. \$\endgroup\$
    – Community Bot
    Commented Mar 5 at 4:45
  • 1
    \$\begingroup\$ The document is quite clear: no ground under the antenna. The this applies to all and any layer. Nothing you learned about multilayer boards seems to contradict that - no ground means no ground. \$\endgroup\$
    – sina bala
    Commented Mar 5 at 8:35

1 Answer 1


Your confusion may be due to the dual meanings of the term "ground plane".

In designing a PCB (not an antenna) it's good practice to dedicate one copper layer to serve as a ground plane. It reduces unwanted RF radiation from the signals flowing on the board, as well as incoming noise from RF sources.

In designing an antenna, the opposite result is desired -- you want it to radiate and receive RF, and for that it needs to be away from ground. That's why the design you chose specifies no ground plane on any layer under the antenna area.

But -- many antennas, such as this one, are designed as monopoles. Think of these as really only half an antenna, requiring some kind of ground plane to serve as the other half. The ground layers on your PCB that are away from the antenna area serve this purpose.

Notice that the reference design has the antenna at the end of a PCB, not embedded in a larger PCB. I think your disappointing results are due to the way you've sunken the antenna area into a notch in a larger PCB. Try removing more of the ground plane along the top edge of the PCB, at least until you reach those headers. It may help some. But the "meander" antenna design is not going to be as efficient as one that spreads the antenna trace out into something closer to a quarter-wavelength at the operating frequency.

  • 1
    \$\begingroup\$ +1. The ground is as important as the "antenna". If you copy a design, it's extremely important to not only copy the shape of the antenna, but the shapes of other conductors in its vicinity. \$\endgroup\$
    – John Doty
    Commented Mar 5 at 17:07
  • \$\begingroup\$ Thank you Mark Leavitt, that was exactly my confusion. So far I've designed a handful of PCBs but none with an antenna - so my use of ground plane was just that - a dedicated layer on a 4-layer board. Hence my confusion when the references mentioned ground planes and the dual meanings. It makes sense now, thanks for your detailed answer. One follow on. I can certainly increase the size of the no-ground region but you mention other shapes. I've read about the inverted F is better in that regard than the meander. Is that one of the ones you recommend? \$\endgroup\$
    – Nollstead
    Commented Mar 6 at 3:24
  • \$\begingroup\$ @user3416569 Yes, the inverted-F is a popular design. It’s basically a quarter-wave monopole with a shunt feed. But those two potentiometers adjacent represent a lot of grounded metal. If you’re redesigning the board, maybe you can relocate the antenna to a clearer area. \$\endgroup\$ Commented Mar 6 at 3:33
  • \$\begingroup\$ Good point, I'll look into that. Thank you again for your detailed answer, it's exactly the help I needed. \$\endgroup\$
    – Nollstead
    Commented Mar 6 at 4:21

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.