Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

How to measure trace impedance

  1. Nov 13, 2014 #1
    Hi, I am working on a PCB that requires controlled trace impedance. I figured out width of the traces and layer stack thickness. How would I verify trace impedance once I get my PCB boards? What equipment do I need?
     
  2. jcsd
  3. Nov 13, 2014 #2

    Baluncore

    User Avatar
    Science Advisor

  4. Nov 13, 2014 #3
    Thank you Baluncore, good info.
     
  5. Nov 13, 2014 #4

    Baluncore

    User Avatar
    Science Advisor

    The solution will depend on the length of the tracks and your budget. If your tracks are short you will have trouble paying for a TDR capable of resolving mismatches. Non-Linear Transmission Lines, (NLTL), have made pulse generator and sampling systems with 100 GHz bandwidth available in the last ten years. They are capable of accurately resolving sub-millimetre discontinuities.

    You may verify your design at less cost by using an RF sweep generator for the frequency band of interest, along with a directional coupler feeding any reflected energy to a sensitive detector.

    You have not identified the track length, impedance, or frequency band of interest.
    Ask more specific questions if you need more information on economic solutions.
     
  6. Nov 13, 2014 #5

    berkeman

    User Avatar

    Staff: Mentor

    What Zo are you designing to? How are you terminating the lines? Forward-termination or back-termination? If back-termination, what is the output impedance of your drive gates? Are these traces multi-drop or point-to-point? What length are they?
     
  7. Nov 13, 2014 #6
    Frequency is 580 MHz, trace impedance has to be ~50 Ohm (Zo), there is a requirement for differential traces as well Zdiff = ~110 Ohm. Trace width is 5mill over 3.5 mill FR-4 (dielectric constant = 3.6 - 4.2). The traces are point to point and average length is 0.85 inch. How can I use RF sweep generator? There is also RF part that runs at 2.4 GHz. I have microstrip line of 20 mill over 7 mill substrate connecting RF amplifier to a 50 Ohm antenna. There is a ground plane below.
    What is the difference between point to point and multi drop traces. I run traces between my processor and DDR2 SDRAM memory. They are matched in length.
     
    Last edited: Nov 13, 2014
  8. Nov 13, 2014 #7

    berkeman

    User Avatar

    Staff: Mentor

    Since they are point-to-point, the driver and receiver are both 50 Ohms, right? So you don't need to add your own external forward termination at the RX device input?
     
  9. Nov 13, 2014 #8
    Yes, both driver and receiver are 50 Ohm. All I have to do is make a 50 Ohm connection between the two. My question is how can I test my boards before we assemble them.
    Thank you for your posts.
     
  10. Nov 13, 2014 #9

    berkeman

    User Avatar

    Staff: Mentor

    With that short of a trace, as Baluncore says it will take a pretty high-end TDR. Plus it will take a HF termination on the blank PCB to verify the Zo of that shore transmission line (TL) trace. You could include a ground pad next to one of the TL ends to let you connect an 0603 or 0405 50 Ohm SMT termination test resistor for testing the blank PCBs, for example. It may be easier to just use a very high frequency oscilloscope and low-capacitance probe to observe the signal quality at the RX device input to look for any ringing.

    What is the circuit? Can you say?

    Alternately, you can do a test PCB that has longer versions of the TLs, and use more traditional methods and a lower-frequency TDR to verify the 50 Ohm Zo.
     
  11. Nov 13, 2014 #10
    The device is Wi-Fi enabled data transmission unit. I am not sure how much I can disclose I am under NDA. It runs in Linux environment and has 2x2 WiFi radio. Its all high speed. I have made one of the PCB manufacturing requirements - test traces on top layer for 50 and 110 Ohm. I know some PCB houses have required equipment to do the test. I just want to make sure I have equipment that will allow me to test PCB myself. I wonder what kind of equipment they use in a PCB house. If I understand right, you are saying that one way to test my traces is to apply sine wave at one end of a trace and verify integrity of the signal at the other end with 50 Ohm terminations on both ends. I might be able to do that. What equipment would you recommend for RF development in general.
    Thank you
     
  12. Nov 14, 2014 #11

    Baluncore

    User Avatar
    Science Advisor

    For UHF and microwave development you can easily spend US$100k on test gear, but you can usually get away with less than 1% of that if you know what you actually need to measure. To cut the cost of test equipment requires access to RF engineering experience. The "black art" of microwave design and testing becomes a "science" as you gain experience.


    If you apply a sine wave at one end of a Zo trace and terminate the far end with a Zo matching resistor, then you will have no termination mismatch and will not get energy reflected from the far end termination. But if your track has the wrong impedance, you will get some energy reflected.
    A directional coupler samples power on an RF line. It separates the direction of energy propagation, so it can be used to measure reflected energy.
    See; http://en.wikipedia.org/wiki/Power_dividers_and_directional_couplers

    By feeding an RF oscillator signal through a directional coupler and a short coaxial cable link to the near end of your trace, (terminated with Zo at the far end), you can measure the reflected signal. Sweeping across the frequency band of interest will test the level of reflected energy. Your system can be calibrated with a termination resistor alone at the end of your coaxial cable.

    For your 2.4GHz RF 50 ohm input, there will be a connector, trace and terminating load. That can be tested by simply “looking” into that port with the sweep generator through a matched directional coupler.

    There are companies such as Minicircuits that make RF modules including VCOs and couplers.
    http://www.minicircuits.com/homepage/homepage.html
    http://www.minicircuits.com/products/Oscillators.shtml [Broken]
    http://www.minicircuits.com/products/Couplers.shtml [Broken]
    Download guides from this page;
    http://www.minicircuits.com/support/literature.html

    Having a handful of modules will allow you to experiment and build your own test rigs for most manufacturing quality control situations.
     
    Last edited by a moderator: May 7, 2017
  13. Nov 14, 2014 #12
    Thank you Baluncore, great info. I will need some time to digest it. My experience with RF is limited. I did a couple of RF designs in the past by strictly following all the design requirements and it helped. This time I am a little worried because design information for this particular device is very limited and I am on my own to figure out how to make it work in the environment. I might have more questions as I go.
    Thank you again.
     
  14. Nov 16, 2014 #13
    Consider using DDR3, its flyby topology is so much simpler and cleaner from a signal integrity perspective. Plus, you may not be able to get DDR2 memory much longer. DDR2 usually requires you to use a signal integrity simulator during design, and scope to verify on the bench. Impedance of the traces themselves is rarely an issue.

    By the way, if you really want to validate your board vendor's trace impedance, a traditional way of doing this is to include a test "coupon" on your board which is a decently long trace with board mount coaxial connector at each end.
     
  15. Nov 17, 2014 #14
    Hi the_emi_guy, I do not think I can include a test coupon. I have limited space on my board. From your experience, if board house tests the impedance and it passes, can I be sure that the PCB is OK? How would you design a board with test and verification in mind? What equipment would you recommend?
    Thank you.
     
  16. Nov 17, 2014 #15
    Test coupon does not have to be on your board, as long as it comes off of the same panel it will be representative. You really don't need to worry about the trace being 55 ohms vs 50 ohms. In my experience, if you tell board vendor you need 50 ohms you get close enough to 50 ohms. Of course all they are looking at is trace geometry, dielectric, and ground plane separation. You have to make sure you don't have random copper pours hugging your traces or anything else that would effect your trace impedance. We once had an EMI gasket sitting on top of high speed traces causing issues. What you do need to worry about are stub discontinuities, loss (depending on how far you are going), discontinuous ground plane etc.
    Best thing you can do for test and verification is to have access for probing all signals you are concerned about. Sometimes this is a challange these days.
     
  17. Nov 18, 2014 #16

    f95toli

    User Avatar
    Science Advisor
    Gold Member

    Do you actually NEED to test the impedance? The fact that you are only running at 580 MHz with short traces and are using FR-4 (which is a rubbish material anyway if you want real control) would suggest to me that the requirements are not that stringent. In most cases it won't matter if the impedance is off by 2-3 ohms and unless you invest a LOT of money in measurement equipment you will struggle to measure the impedance with an accuracy better than that anyway.
    Also, unless you've really messed up when you designed the traces they should be very close to the design value: if you are unsure you can just look at some test data from the maker of the laminate and just use the same dimensions as them for your transmission lines (unless you are using a board with multiple crossing signal layers).
    Hence, I agree with what was said above: a generator and an oscilloscope will tell you if the signal integrity is OK, don't worry too much about the impedance.

    For the record: I have no formal training in MW design but I do design simple PCBs (sample holders etc) for my experiments, we typically work between 4-8 GHz and I design the lines to be "flat enough" up to about 12 GHz or so (and I DO have the measurement kit needed to test them). I basically use a "cookbook" approach (combined with some Sonnet simulations) and so far all my designs have worked reasonably well. Hence, this type of design is not nearly as difficult as it seems; and I've learned that as long as I don't try to do anything too exotic there there is no need to worry.
     
    Last edited: Nov 18, 2014
  18. Nov 18, 2014 #17
    Thank you guys for your answers, I think I feel a lot more confident now. The reason why I focused on the trace impedance is because it is one thing I never had to deal with and I do not have any experience with. I looks to me if I do my math, figure out all the geometry of the traces, and require the board house to verify the impedance the PCB will be OK. I will try to add test points to my signals of interest. Do you have any recommendation on how to add test points to high speed lines, basically how not to make those connections antennas?
     
  19. Nov 18, 2014 #18

    Baluncore

    User Avatar
    Science Advisor

    You are on the right track.

    You do not want to ship boards that are “deaf” or “dumb” at RF. So first calculate the critical PCB parameters and specify reasonable bounds on impedance that can be met by the PCB manufacturer. Specify the PCB's RF input sensitivity and minimum output power to comply with the standards. You can then quickly test power, sensitivity and/or BER in the finished product. That tests functionality without the need to measure detailed internal diagnostic parameters. A good product will be able to self test it's critical performance parameters following manufacture.

    Where impedance is critical you are better to use one or more matching components that can be adjusted following assembly than to reject boards due to difficult trace impedance control. There is a trick available, by deliberately slightly miss-matching the line driver and receiver, the trace can be made at the geometric mean impedance of those elements. PCB RF performance will be more consistent because variation of mismatch at one end will tend to cancel that at the other. In the extreme situation this approximates a quarter wave transformer.

    UHF and microwave power is expensive to generate so good economy by impedance matching is a better investment than generating higher initial levels. Impedance matching really only becomes critical when low receiver noise or significant power is involved.Transmission lines on cheap PCB are not usually a problem, but when making resonant microwave elements from PCB traces things become more difficult and require better dielectric material with lower loss. That is because, if the element has a Q of say 20, the circulating energy will suffer 20 times the loss.
     
  20. Nov 20, 2014 #19
    Thank you guys for your replies.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: How to measure trace impedance
Loading...