• State Resolved
  • Locked Locked
  • Replies 5 replies
  • Subscribers 16 subscribers
  • Views 805 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.

CC1101 - Corner in the balun and impedance measurement

Stefano Infante
Expert 2320 points
Other Parts Discussed in Thread: CC1101

Hello,

I have two questions for you RF experts, and hope you can help me again.

In the design of my revised board the PCB engineer is thinking about putting a "corner" in the balun section of CC1101. To be more accurate, we have the same exact RF section than the reference board (at 433 MHz), but the very last capacitor (C125 on the CC1101 datasheet) is turned 90° left, in order to save board space by inserting the antenna on the left side instead of straight after the balun. Do you think this could be acceptable or is there any reason to go back and think again about this issue?

The other question is about the impedance measurement. We are using a software which, according to some parameters, gives us the exact impedance of a network. What do we have to expect in order to optimize our design? I see that at 433 MHz the balun impedance should be 116+j41 (datasheet): is it the value I should look for?

Thanks in advance,

Stefano

  • 0
    TI__Mastermind 39860 points

    Stefano,

    Turning the last capacitor (C125) 90 degrees left will not cause any problems. What is important is that you lay out the balun symetrically wrt to RF_N and RF_P.

    Measuring the impedance is not straightforward, but the differential impedance from the RF_N/RF_P pins towards the antenna should ideally be 116+j41. If you follow the reference design, both component values and component placement (except C125 in your case), there should not be any need for measuring the impedance.

  • 0 in reply to Sverre
    Expert 2320 points

    Sverre,

    thank you very much for your help.

    Regarding the impedance measurement issue, the problem is we have to change the W/H ratio, as our board will be a 4-layer one. So my answer is whether or not we can check the evaluated impedance against the 116+j41 reference.

    Thanks again,

    Stefano

  • 0 in reply to Stefano Infante
    TI__Mastermind 39860 points

    As long as the distance to the ground pane is 0.25 mm or more you can use the CC1101EM reference design as is.

    The only part of the reference design where there is a 50 ohm line is from the last capacitor towrds the SMA connector. Changing the W/H ratio will change the impedance. As a rule-of-thumb: for epsilon=4.8 (common for FR4) a W/H = 1.8 gives 50 ohm. Note that for short tracks (less than one-tenth of wavelength) the line can be considered lumped circuit 

  • 0 in reply to Sverre
    Expert 2320 points

    Sorry, this is my fault. I was wrong in explaining what we are doing.

    We are trying to change W and H, having a 4-layer FR4 PCB, in order to keep the W/H ratio similar (equal) to the one in the reference board.

    Another misunderstanding between me and the PCB designer is I talked of total impedance (which should be 116 + j41, and is guaranteed by following the reference board design), while he intended the line impedance (which, as you are saying, should be about 50 ohm in the last part of the circuit.

    So the rules we are following are:

    - place the C125 capacitor in a "corner" way, in order to save board space, while maintaining 50 ohm between itself and the SMA connector;

    - given a value for H (which will be the thickness between the first two layers) higher than 0.25 mm, change the width of the matching network lines in order to keep the W/H ratio as similar as possible to the W/H ratio on the reference design.

    My last question is: given these two rules, is there anything more we should take account of?

     

    Thanks again, your help has been very useful.

    Stefano

  • 0 in reply to Stefano Infante
    TI__Mastermind 39860 points

    Stefano,

    You should follow your "rule 1"

    As for "rule 2" you can keep the balun (PCB tracks, component values, component placement) equal to the reference design and there is no need to change the width. In our experience we have not seen any degradation in performance as long as the height to ground is more then 0.25 mm. We have made a 4 layer PCB for CC430, which is the same radio as the CC1101, and we used the same balun for the 4 layer CC430 PCB and the 2 layer CC1101 PCB