nrf51422 decoupling capacitors

RE: nrf51422 decoupling capacitors

Fredrik Sundt Brynhildsvoll — Wed, 02 Mar 2016 11:39:50 GMT

I am sorry, I misunderstood your question. Yes you need a ground plane below the matching circuit of the antenna. With a 4 layer pcb it is recommended to use the layer furthest apart from the matching network as a ground plane and keep the inner layers restricted (no ground or lines). This is done on nrf51 dk. I believe you will benefit from looking at this question. You should also see the pcb guidelines for the nrf52 chip.

RE: nrf51422 decoupling capacitors

tuv0k — Wed, 02 Mar 2016 10:52:59 GMT

Maybe I misunderstand something, but shouldn't the trace between balun and PCB antenna be 50ohm impedance controlled? In that case, distance between top layer and gnd plane matters as well as width of the trace.

RE: nrf51422 decoupling capacitors

Fredrik Sundt Brynhildsvoll — Wed, 02 Mar 2016 10:24:30 GMT

I am not sure if I understand your first question, but the thickness of the layers is correct and the dielectric properties are too.

Second question: It is not necessary, but good practice. Generally the size of the ground plane is proportional to the performance of the antenna. The bigger the better.

RE: nrf51422 decoupling capacitors

tuv0k — Wed, 02 Mar 2016 09:53:36 GMT

Thank you for very helpful answer! Is the stackup of nRF51-DK defined in Altium PCB accurate? (imagizer.imageshack.us/.../Cm7w81.png) Would it be necessary to pour GND on the BOTTOM layer?

RE: nrf51422 decoupling capacitors

Fredrik Sundt Brynhildsvoll — Wed, 02 Mar 2016 09:01:49 GMT

Hello,

the approach of connecting grounds together in a local plane and then connecting this again to the global plane in one point will generally generate less noise in the ground plane. But due to the long lines there will be an increase in the inductance between the chip vss pins and the ground plane. For a microcontroller without an radio this is usually not a problem and it is good practice. This is not the case for our chips.

The antenna use the ground plane as a reference and a relatively small inductance will at 2.4GHz function as an open circuit, meaning the antenna will have problems seeing the ground.

So there is a trade off between the noise in the ground plane and how good the RF performance of the design will be. If your system is not very sensitive to noise in the ground (because you have sensitive analog devices connected) I would recommend to use the guidelines in the product specification.

We have also written a tutorial which describe general PCB guidelines for the nrf51 chip. You can pick up a lot of tips on how a circuit should be designed to be used with high frequencies. It is found here.