• State Resolved
  • Locked Locked
  • Replies 5 replies
  • Answers 1 answer
  • Subscribers 51 subscribers
  • Views 608 views
  • Users 0 members are here
Support feedback
Options
Options
Related

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.

Original question:

CC2650: launchpad rev 1.3 return loss on port P11

CC2650: Launchpad ref design stack up + antenna question

Raghu Tumati
Intellectual 720 points
Part Number: CC2650

Hi 

I've been looking at the Gerber files for the cc2650 rev 1.3 launchpad a bit before I start my custom board design using the cc2650 for a bluetooth application. I am also designing the board with a PCB antenna similar to that on the launchpad. 

I have a question about the antenna design and stack up. I realize that the IFA antenna on the launchpad is a lambda/4 monopole which forms one half of the dipole antenna. The other half of the dipole (lamda/4)  is formed on the ground plane of the launchpad. Now from the Gerber files I see that layer 2 and layer 4 are used as complete ground planes with no routing or components. 

Q1) is the other half of the dipole formed on layer 2 or layer 4. Why do we have two complete uninterrupted ground planes in the stack up? Would just one not be enough.

I initially thought that layer 2 is used as a reference layer for the 50Ohm GCPW transmission lines on the top layer and other return paths and layer 4 is for the antenna but I am not sure. How is it decided which ground plane will be used for the other half of the antenna dipole?

Q2) Say I have the following stack up.

Layer 1 is RF traces + components + routing .

Layer 2 is an uninterrupted ground plane.

layer 3 is a uninterrupted power plane.

Layer 4 is ground plane + routing. 

Would this stack up also work? Here I would guess the other half of the dipole antenna will be on layer 2. 

I would appreciate any feedback. This would definitely help me understand more about RF board design. 

Thanks

Raghu

  • 0
    TI__Mastermind 33190 points
    HI,

    A1) Correct that the other half of the dipole design is formed in the GND layer. For the antenna operation it would be sufficient with just one GND layer. The majority of antenna test boards from several antenna vendors are just single sided one-layer designs. Ideally, the GND layer for the antenna should be the top or bottom layer so the radiation from this layer will not be interrupted by other traces. But for the chip for good harmonics, return GND loop currents, it is better to have the GND on layer 2. So the layer 2 GND is mostly for the chip and layer 4 GND is mostly for the antenna. Since we use the lowest cost of vias which is through-hole, the antenna GND layer will be a combination of both of these layers.

    A2) Your stack-up would be fine. I personally, would also route on layer 3 since you do not need to have a complete power plane on the whole PCB. The power routing should be done first and have the highest priority. Then other "noisy" signals can be routed and encapsulated between the two GND layers (Faradays cage effect); this would help to keep the radiated emissions as low as possible. The antenna GND would be a combination of layer 2 & 4. I would also add GND vias around the edge of the PCB to try to unify the GNDs.

    Regards,
    Richard
  • 0 in reply to RGW
    Intellectual 720 points

    Hi Richard

     Thanks for your reply. This really helps. However I would like to follow up on a few comments you made to further solidify my understanding 

    "Ideally, the GND layer for the antenna should be the top or bottom layer so the radiation from this layer will not be interrupted by other traces"

    When you say "radiation from this layer", do you mean radiation from the ground layer that mirrors the other half of the dipole? I didn't think a ground plane could radiate. For radiation there has to be a potential difference but its a solid ground plane. Or does the formation of the other half of the dipole cause some oscillating currents magnetic fields and voltages? 

    "will not be interrupted by other traces". Do you mean traces in its adjacent layers? So if I have a antenna ground plane on layer 2. And layer 3/4 is used for routing, these traces would interfere with radiation from layer 2. 

    Two more follow up questions 

    1. Does the antenna ground plane always need to be a solid ground plane?

    2. Any reason why on the launchpad, layer 3 does not have a ground fill? 

    Thanks

    Raghu

  • 0 in reply to Raghu Tumati
    TI__Mastermind 33190 points
    Hi,

    Yes, the mirroring effect caused in the ground plane of the antenna plays a significant role. This can be tested by reducing the size of the GND plane and the radiated efficiency will be reduced. This is valid for all types of monopole designs. The formation of the GND plane will contain oscillating currents, magnetic fields.

    The GND plane does not have to be solid for the antenna. Refer to Marconi Antenna as an example. A solid GND plane is advantageous for return loop currents and lowering emissions but this is for the other electronics on the PCB.

    For the LP designs, we try to keep the metal plane symmetry balanced on the PCB stack-up. i.e. similar metal amount on L1+L2 to L3+L4. This is not a primary rule but just helps reducing the risks of warping the PCB.

    Regards,
    Richard
  • 0 in reply to RGW
    TI__Mastermind 33190 points
    Hi Raghu,

    There is a very good app note describing RF simulation and this also covers antenna simulation to a certain degree:

    www.ti.com/.../swra638.pdf

    Regards,
    Richard
  • 0 in reply to RGW
    Intellectual 720 points

    Hi Richard

     Thank you! Thank you so much for your patience and detailed explanation. I really appreciate it. 

    -Raghu