Ground plane under antenna matching components?

[Lauri Jämsä]

We're designing a new revision of our open source sensor beacon platform: http://ruuvi.com

Just want to make sure I got this right. nRF51/2 Reference PCB Guidelines states:

A PCB with a minimum of two layers, including a ground plane, is recommended for optimal performance. On PCBs with more than two layers, put a keep-out area on the inner layers directly below the antenna matching circuitry (components between device pin ANT and the antenna) to reduce the stray capacitances that influence RF performance.

Questions:

1. If we put keep-out areas on inner layers, should we leave the GND copper on bottom layer anyways? Our PCB is 4-layer 1.6mm FR4.
2. In case of thin 2-layer PCB (flex for example), should the bottom layer have copper under the matching components or not?

If in case of multilayer PCB (more than 2) the copper plane should be there on bottom layer, I think you should mention this on your PCB guidelines. And also specify how thick the PCB has to be so that GND plane on bottom layer won't cause the stray capacitances that may have influence to the RF performance.

HW & SW source files: https://github.com/ruuvi/

[bjorn-spockeli]

1. Yes, the bottom ground layer is needed in order to shield the matching network. Keep-out areas apply to signals, ground and power planes in the inner layers . A general rule of thumb is to use the layer furthest away from the matching network as ground.

2. Yes, the bottom ground layer is needed in order to shield the matching network.

I will look into the recommended PCB thickness and update my answer.

Update: Nordic layouts are recommended for 1.6mm to 0.8mm PCB thickness. Anything thinner requires tuning of the matching network and possible degradation of performance.

Best regards,

Bjørn

[Lauri Jämsä]

Great, thanks for this info.