• State Resolved
  • Locked Locked
  • Replies 5 replies
  • Subscribers 17 subscribers
  • Views 3489 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.

Right SMA trace width for low-power board?

kazola
Guru 18595 points

Hi all,

from this application note I have extracted the following figures, not related to my current work :)

However, as you can see, in all of them the trace from / to SMA antenna plug is drawn as wider than the rest. This is not my work area but I want to design a low-power board as well as possible. Hope you can help me with some questions! :)

In the board I'm designing, I'm working at 868MHz. All the components are connected by 0.3mm traces. I know the impedance of the previously mentioned SMA trace is related to its width, which will be probably higher than 0.3mm. In my board, just after the SMA trace there is a 0603 inductor which is part of an impedance matching network. Thus, when drawing my board in EAGLE, I find that the width of the SMA trace should be kind of assymetric, since the SMA side is much wider than the pad of the 0603 component I want it to be attached to.

So, my questions are:

  1. Which is the trace width you use to employ for SMA traces? Since the SMA center pin is considerable in size, I guess for maximum energy transfer the trace coming out of it has to be bigger, as in the pictures I attached.
  2. Which is the correct way to design this? Keeping the SMA trace as short as possible to make it affect the impedance matching as few as possible, or allow the SMA trace to have a length of 1cm for example and re-do my impedance calculations taking this into account? The value of the 0603 inductor is known but right now I do not have the paper here :(

Ok, eagering to know your opinions! I have searched the forum for something similar to this but I was not able (yet) to extract related information, if any :)

  • 0
    TI__Mastermind 21190 points

     The impedance of the traces depends on the PCB substrate and dimensions of copper traces. You can use AppCad(free SW) to determine the trace dimensions for any impedance you are designing for.

    Once you have the design, you can simulate it in an RF simulator and tweak the it for required performance.

  • 0 in reply to FI
    Guru 18595 points
    I know this, thanks. However, my questions are a bit more specific.
  • 0 in reply to kazola
    TI__Mastermind 27145 points

    In your picture, the output of the filter (L2/C3 Juction) should be a 50 ohm impedance.

    Yes, you are right. The trace width should be wider than the component pads (for example SMA Connctor Pad). But in some cases it is impracticable to design a wider tarce width because of PCB stcak-up. If there is a little variation in the trace widths, it creates a little missmatch but it doesn't affect the performane that much.

     

    If your application requires exact match then you need to work on the PCB stack-up and material to get the required trace width to match (wider than) to the component pads. If possible, better to use shorter trace lenghs.

     

    Thanks,

    PM

  • 0
    Expert 1445 points

    Hello,


    1.  The SMA microstrip trace width can be easily calculated knowing the PCB dielectric constant, PCB thickness and trace metal thickness.  For example, if the dielectric constant is 4.6, PCB thickness is 20 mils, trace thickness is 2.1 mils then  the required 50 ohm trace width is approx 35 mils.  I used Avago AppCAD for that calculation.  AppCAD is a free download from Avago.  (Sorry but I switched to mils and you were using cm.)

    2. Keep the trace lengths between your matching components as short as possible.  Position the parts as close together as your MFG people allow.  Otherwise, your 50 ohm line will be part of your matching network.  For example, if you were using the schematic you pasted above, position C2, L2 and C3 very close to the 20 ohm circuit input or output.  Once you've matched it to 50 ohms, then use your 50 ohm microstrip line to the SMA connector.  These are quick, general guidelines.   


    I would be happy to take a quick look at your PCB layout after you've placed the parts.  You could email it directly to me if desired.

    Regards,

    Eric Hooker

    RF Consultant

    EHooker-RF@msn.com

  • 0 in reply to Eric Hooker
    Guru 18595 points

    Many thanks to everybody!

    Regarding Eric's answers:

    1) Yeah I know Avago AppCAD, very nice! However, in my case trace thickness is not 2.1 mils but 1.37 mils = 35um. PCB Thickness is 1.5mm = 59 mils. Er = 4.6. This makes my SMA traces to be around 2 mm = 82.5 mils for be even close to 50 ohm. Argh!

    2) Thanks for your advice! :)

    Ok, just sent you an e-mail. I'm closing this thread! Thanks to everybody!