4
\$\begingroup\$

I've found a lot of RF chip antennas that in their datasheet provide a reference/test PCB layout with RF results. This PCBs have antenna mounting position and a RF line surrounded by GND plane.

Are this GND planes necessary to antenna to operate or they just report test board layout?

I ask this becouse my board is smaller than 30mm and top ground is splitted becouse components mounting, most reference board have 50mm lenght and solid ground plane.

Here's some examples of what I say: enter image description here Datasheet link: http://www.johansontechnology.com/datasheets/antennas/2450AT42A100_v2.pdf

\$\endgroup\$
  • 1
    \$\begingroup\$ I am interested in your results and experiments? Can you update your question and add your experience and conclusion? \$\endgroup\$ – abhiarora Oct 28 '17 at 17:27
5
\$\begingroup\$

Are this GND planes necessary for the antenna to operate or they just report test board layout?

Yes and no. In your example, their test fixture shows a connector (probably SMA), surrounded by ground plane, and a feedline leading to the chip antenna, which is outside of the ground plane. This is assuming the PCB is double-sided, and probably 4 layers or more. This is a "standard" test setup, designed to maximize performance. An ideal PCB could be shaped this way.

What doesn't matter is the connector and location of the feedline. But changing the position of the antenna relative to the ground plane, and/or changing the size/shape of the ground plane, will all affect the performance.

If possible, using a layout similar to the illustration will likely give results similar to theirs. Just be aware that if you start modifying anything, it will change the results, and you'll end up having to perform an impedance compensation requiring very expensive lab equipment. Changing the position of say, the antenna by 1mm could make a significant difference. Dimensions must be exact for high-frequency use (MHz and GHz.)

You cannot operate well without a ground plane at all. The many vias stitch both outer layers together (ground of a four-layer PCB) to eliminate any coupled RF energy from penetrating the PCB. For a receiver, it is possible to do single-side ground plane, and for some circuits this is fine, even with broken ground plane. For a transmitter, not shown is even more vias, placed less than a tenth of the RF wavelength apart in the middle of the copper, to prevent induced currents from creating gradient voltages in the copper itself. Not an issue for a receiver, but a great concern when dealing with high-impedance signals near a transmitting antenna.

\$\endgroup\$
3
\$\begingroup\$

The point is that your feedline is labeled 50Ω, which is a property you can only achieve with a PCB line in combination with a ground plane.

So, from an antenna point of view, the ground plane is probably insignificant (depends on the antenna, actually), it's important that whatever you use to feed the antenna is impedance-matched.

What your diagram shows is typically known as coplanar wave guide, by the way.

\$\endgroup\$
0
\$\begingroup\$

It's not required in all cases. In principle, there must be a return path for current. In case of microstrip based structure, this return path is through ground plane beneath the feed-line and patch antenna. While in case of co-planar structure ( like CPW line) no ground plane in needed below that chip antenna.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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