• State Resolved
  • Locked Locked
  • Replies 9 replies
  • Answers 2 answers
  • Subscribers 30 subscribers
  • Views 1165 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

IWR1843: Antenna design for custom PCB

c64
Intellectual 480 points
Part Number: IWR1843
Other Parts Discussed in Thread: IWR1642BOOST

Hi,

We're in the process of designing a custom PCB for an IWR1843 application, and I have a few questions regarding the antenna design. First of all we're quite cramped on space, and since we don't need any angular information for our particular application, we will have 1 TX and 1 RX antenna. Furthermore, another restriction, is that the PCB will be 30 mm in diameter. So based on that, I'm wondering about the following:

1. On the IWR1843 BOOST eval board, it seems like there are two antenna patch strips on both sides of the RX antennas connected to GND. Why is that, and what is the consequence of not including them?

2. Due to the geometry of our PCB, we were thinking of curving the RX and TX antennas to follow the curvature of the PCB, instead of having them as straight lines. Will this be a problem? Since we're not interested in any angles, and just using one antenna of each, I assume there would be no phase issues. Am I correct?

3. On the evaluation board there is a pretty large GND area exposed under parts of the antennas. Is there a reason why this is exposed and not designed as a layer in the middle parts of the PCB? Is there a consequence if incorporating this as an inner layer, and not exposed? Since we are pretty cramped for space, we would like to use the other side of the PCB for other components.

Thanks!

  • 0
    TI__Mastermind 23625 points

    Hello

    Have you had a chance to look at the following app note?

    TI mmWave Radar sensor RF PCB Design, Manufacturing and Validation Guide

    We will get back with more detailed responses , for the  #1, #3 are antenna simulation based improvements.

    For #2 you risk rotating the E and H planes which may combine/cancel with the one from different patch if the two patches are rotated wrt to each other.

    Regards

    Vaibhav

  • 0 in reply to Vaibhav Mahimkar
    Intellectual 480 points

    Hi,

    Thank you for the prompt answer. I'm looking forward to the more detailed response. 

    As for #2: I don't have any CAD drawing skills, so had to make a very course sketch in PowerPoint that I'm copying and pasting, just to illustrate what I mean. Obviously in the physical PCB layout, the Rx and Tx will be more symmetric and so forth, but the figure below is just to show my initial idea to make room. I've been measuring the eval-kit, and we might be able to incorporate straight antenna patch strips, but in case we are not able to do that, would we still experience the effects you mention in your response, given my simplistic illustration? Would it be better if the Rx antenna would curve in the counter-clockwise manner, while the Tx in the clockwise manner? Or would there be too much uncertainty to know at all? If we need a curvature of the antennas, any first-order ideas of how they should be formed wrt each other?

  • 0 in reply to c64
    Intellectual 480 points

    Hi again,

    I don't think my pasted figure came out correct, so I'm trying once more:

  • 0 in reply to c64
    TI__Mastermind 25805 points

    Hello,

        For these kind of customization antenna need to be redesigned. Antenna need to be redesigned based on the Field of view, max distance, Bandwidth required, beam pattern required, Antenna gain etc. This kind of change will change adversely affect the antenna radiation pattern. Arbitrarily we cannot change the structure of antenna without any effect on the Antenna performance. This must be designed and studied using  a 3D EM simulator and then optimal solution need to be arrived yet. 

    If you want to alter the beam pattern you could use a lens as well. You could review some of the discussion on this topic here.

    For the above questions please find my comments below

    1) These are dummy antennas, It helps to match the parasitic, you could review the role in the e2e post here, 

    2) Definitely there would be effect on the Antenna radiation pattern, As mentioned above, without the simulation it's hard to comment on the effectiveness. There could be effect on he polarization as well If the Tx and Rx Antenna are not identical. 

    3) Could you please elaborate bit more pictorially which regions specifically referring to? Ground plane is part the antenna design for the intentional radiation in the the given desired direction. Also solder mask is exposed for the ground and Antenna regions as it would affect the impedance of the  RF traces and Antenna.

    Thanks and regards,

    CHETHAN KUMAR Y.B.

  • 0 in reply to CHETHAN KUMAR Y.B.
    Intellectual 480 points

    Hi,

    Thank you for your answer. I think we will try and make space for the antenna topology found on the evaluation board (straight antennas, and in parallel). As for #3, I have home office these days, so I only had access to an IWR1642BOOST for the pictures (the IWR1843 would be similar). It has been in a few field tests, so I apologize for the rough treatment. Anyways, below I've attached a picture of the front and back sides. So my original question was why is this GND plane exposed, and not put in a middle layer. We want to utilize as much of the PCB area as possible, so ideally we'd like to put the GND plane in a middle layer, leaving the bottom part of the PCB available for other components. I also notice that there is no GND plane exposed for the RX antennas. Why is that?

    Thanks!

  • 0 in reply to c64
    TI__Mastermind 25805 points

    Hello,

       This ground exposure is mainly to provide heat transfer mechanism.

    For the additional thermal mitigation, plan was to have heat from the device underneath the package on the bottom side of the board transferred to the exposed copper area and suitable heatsink that could be connected to this area to dissipate the heat. However were didn't had to exercise this option as power dissipations were under control. Hence you should be able to use this area for other components as well. 

    Thanks and regards,

    CHETHAN KUMAR Y.B.

  • 0 in reply to CHETHAN KUMAR Y.B.
    Intellectual 480 points

    Hi again,

    Thank you so much for your answers. Just a quick question. Would there be an issue if I placed components directly on the backside of the PCB from where the antennas are located?

    Thanks!

  • 0 in reply to c64
    TI__Mastermind 25805 points

    Hello,

        In principle you could keep the components on the back side of PCB from where Antenna are located, however while routing the signal you may need some vias, and If these vias are micro-vias from the bottom side without affecting the Antenna then it's fine. However if you use through vias then it would affect the Antennas, transmission lines that would be detrimental, Hence, best it could be avoided.

    Thanks and regards,

    CHETHAN KUMAR Y.B.