• State Resolved
  • Locked Locked
  • Replies 4 replies
  • Answers 1 answer
  • Subscribers 53 subscribers
  • Views 940 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:

CC1352P: Antenna design consideration with FR01-S4-224

CC1352P: Impedance routing of ANT MN

Den L
Intellectual 990 points
Part Number: CC1352P
Other Parts Discussed in Thread: CC-ANTENNA-DK2

Hello, 

I have a question regarding Impedance Routing of the CC1352 Antenna traces. In this thread from a while ago - https://e2e.ti.com/support/wireless-connectivity/sub-1-ghz/f/156/t/842724 I have asked about the width of the tracks which were used in LAUNCHXL-CC1352P1. 

The answer was:

"The trace width is 150 um for all the RF front-end routing to the "50" ohm point/switch. 
Then the "CPW Ground" trace (gap/width/gap) is 500 um / 300 um / 500 um or 150 um / 250 um / 150 um. Both give approx 50 ohm characteristic impedance."

After comparison with the actual design I have a few questions which are still confusing me:

1. I assume that the routing should start with 100 Ohm Diff impedance. However, it doesn't feel like this in the Dev. Kit. design. The track width is 150um but separation varies on all ANT channels, i.e. it is not constant how it should be in diff. routing.

2. I assume that after C489, L336 the impedance should be 50 SE? (which is 150um in your stack..) 

3. The track width already changes after C36 to 250um, i.e. what should be 50 Ohm Coplanar. However, at the bent point to RF SW the GND/SIG separation is not constant as well...

Does it make no difference if I route everything with 50Ohm SE?

In my design I started with 100 Ohm Differential until the MN (I also have relatively long traces until MN... ) and continued with 50 Ohm SE everywhere else until RF SW where I used 50 Ohm Coplanar. After my design came from the assembly, I then connected it through JSC to your CC-ANTENNA-DK2 Kit and the performance seems to be almost the same. So, I am a bit confused, what is the more correct approach, if I was just lucky or ..?

Thanks in advance!

Regards,

Den

  • 0
    TI__Guru**** 317180 points

    Note that a trace has to be > 1/10 of the wavelength for the RF frequency used before the trace will behave like a transmission line. 

    Note that the output of the balun should not be regarded as a 50 ohm point, in this case only the input to the switch (and onward) is a 50 ohm point. 

    Due to this the routing between the components could have a bit "random" line width, sometime the line width is selected to fit to the footprint of the components. 

    A long routing as to the first component in the balun as you have here is not recommended since the traces represent a impedance and cause a phase shift that could cause the PA to not see the recommend impedance. I assume that you checked the harmonics also when you checked the performance on your board. 

  • 0 in reply to TER
    Intellectual 990 points

    Thanks for the reply!

    That would make traces of ca. 1.6 cm for 1-Sub and 0.6 cm for 2.4 GHz. In case of 2.4 GHz on the LAUNCHXL-CC1352P1 the traces are a bit longer than 0.6 cm before they are matched to 50 Ohm..

     

    I basically didn't know that balun doesn't need traces of 50 Ohm. Additionally, the pin naming on antenna pins as _N & _P confused me a bit, cause in general it implies that you have differential routing. (typically 100 Ohm).

    I know that these long traces are not optimal, but my PCB has a very narrow form factor, I can't put them closer, otherwise I just don't have space to route it. I will give it another try to move it a bit closer in the next design, but this is quite "squeezed" as is. Also, I am a bit afraid of a risk of cross-talk in case I have all the MN circuit lumped together. Mainly the influence of the 2.4Ghz.

    Kind Regards,
    Den

  • 0 in reply to Den L
    TI__Guru**** 317180 points

    With regards to 50 ohm tracs etc: The easiest would be ot use the same trace widths as the ref design with exception to the track towards the antenna which, to be safe, should be regarded as a 50 ohm track. 

    RF_P/RF_N are differential but not 100 ohm.

    If you are size limited you can look into the IPCs available, you can find a full list here: www.ti.com/.../swra640

  • 0 in reply to TER
    Intellectual 990 points

    Basically, I got the main points, hence the questions are answered and the thread can be closed. 


    Thanks for the help!