This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

RF multilayer board for CC2520 design

Other Parts Discussed in Thread: CC2520, CC2591


Is there any application note that details on RF design for a multilayer board using CC2520??? We plan for a 6 layer board

What are the precautions to be taken?? How to ensure a low loss RF path ?? Is there a tool to support such designs for CC2520

  • Hi Rakesh,

    If you will be using a 6-layer board then start with the reference design for the 4-layer board. Try to maintain the layer thickness between the top layer (layer 1) and the GND layer (layer 2) with your 6-layer design as used in the standard 4-layer ref design; if the same layer thickness cannot be achieved then layers 2 and 5 can be left empty underneath the radio region to help make a similiar layer thickness as used in the standard ref design.

    i.e.  std 4-layer ref design -> 6-layer design

    Layer 1 -> Layer 1

    Layer  2  thickness -> Layer 2 + Layer 3 thickness


    Layer  3  thickness -> Layer 4 + Layer 5 thickness

    Layer 4 -> Layer 6

    This can be done to maintain the symmetry around the core of the pcb otherwise the layers can be just copied layer 1 to layer 1 etc and this will give an assymetrical design and the radio discretes might need to be tweeked if the layer thickness has changed too much from the standard ref design. If the layer thickness cannot be maintained then it could be a solution to have a matched filter balun part instead of the discrete network since these are usually less sensitive for layer thickness change.

    To minimize the RF losses, the 50 ohm lines can always be adjusted to suit the layer thickness change.  If the tracks are too thin then just keep with the minimum track width and place the components as close as possible.



  • Hi Rakesh,

    I would suggest reading this document:, and of course to study the CC2520 reference design.

    For 6 layer design the only requirement is that the ground plane is directly underneath the layer with the RF signals (ie. 1:RF, 2:GND, 3:VDD, 4:signal, 5:signal, 6:signal). If you have RF traces which are more than a couple of mm long it makes sense to make sure they have 50 ohm impedance. TX-line is a very nice and free tool to calculate transmission line impedance.

    I you are planning to use PCB antenna I would recommend either DN007 or AN043.


  • Hi,

     I checked the CC2520Em reference design . It is a 2 layer board. Which is the 4 layer reference design files for CC2520 ??

    Is it the CC2520+CC2591??

    Does the balun design with discrete also vary with the board stack height especially the track line inductance??

  • Hi,

    The CC2520 CC2591 Ref Design ( is a 4-layer, 1.6mm thick EM board design; the distance between layer 1 & 2 (GND ref) is 175um in this design. If following this ref design which uses discrete inductors then this is less sensitive for layer thickness changes but still recommend to use a similiar thickness since the Q in the discrete inductor can change depending on the distance to the GND plane. This is a lot less sensitive than using T-Line approach.

    CC2520 Ref Design ( is a 2-layer, 0.8mm thick EM boards design; the distance between layer 1 & 2 (GND ref) is 775um in this design. If following ths ref design then the distance between layer 1 and 2 must be followed since this design utilises T-Lines (integrated inductors into the pcb). The T-lines are dependent on the distance to GND.

    Depending on your 6-layer stackup, you can choose either of the designs. If there are alterations in the layer thickness compared to the ref design then keep with the discrete version to reduce any risk.



  • Hi,

    Based on the suggestion above I would like to design a 4layer rather than the 6 mentioned before. I want to adopt the 4 layer (CC2591) design to CC2520 . Thickness of 0.775u Dielectric

    I have followed a balun design suggested in

    "" in order to avoid dependency on layer thickness.

    I have also attached the schematics ... Is it correct???Please verify .... Doesnt this need DC blocking capacitors..... Will the performance be on par with the Transmission line design (CC2520 EM design)....

    By the way CC2591 EM Is it mandatory for ground plane to have 18micron thickness?