PCB design: Long analog signal trace

Discussion in 'Analog & Mixed-Signal Design' started by DreeOlee, May 11, 2018.

  1. DreeOlee

    Thread Starter New Member

    May 11, 2018
    3
    0
    Hello,

    I have an analog differential signal. This signal has to be transported over a 20cm PCB trace.
    I want to place the instrumentation amplifier near the analog differential signal and than transport the analog signal (0..3.3V) over the PCB.

    To minimize (EMC) influence from outside, what is the best practice for:
    1. Trace width (wide or small)
    2. Ground plane offset distance

    Thanks.
     
  2. MrChips

    Moderator

    Oct 2, 2009
    16,503
    5,065
    Welcome to AAC!

    Use coax cable such as RG-174/U.
     
  3. DECELL

    Member

    Apr 23, 2018
    96
    19
    I am assuming that your analog signal is low frequency and the input current will be uA?
    So go small on the trace width and keep the traces for this signal as close as possible. Use a plane underneath (pink) and arround trace pair (green), use plenty of vias to make a cage. For best performance connect this plane to local ground at the measuring end only.

    Or (as the Mrchips says) run the signal in a cable. A shielded twisted pair (you know, the ones who live next door!) cable will do.
    Tie the cable shield(s) to ground at the measuring end only . If not you may generate an earth loop and make things worse.
    The wider the effective apperture of any loop the more lines of unwanted magnetic flux will cut through it. More flux, more induced intereference.
    upload_2018-5-11_15-59-53.png
     
  4. DECELL

    Member

    Apr 23, 2018
    96
    19
  5. crutschow

    Expert

    Mar 14, 2008
    19,363
    5,396
    Yes, for a differential signal you want shielded-twisted-pair, not coax.
     
  6. ebp

    Well-Known Member

    Feb 8, 2018
    1,422
    477
    I'm not totally clear on intent here. The objective is to run the output signal from the instrumentation amplifier via the 20 cm trace? Are you concerned with radiation from that trace or coupling into it from outside sources?

    If the maximum frequency content (i.e. considering the frequency spectrum, not the repetition rate) is less than a few megahertz, the trace width really won't make much difference at 20 cm. Guarding the trace on both sides with well-grounded traces has some merit and can certainly be helpful if you have to have parallel traces that carry fast analog signals or digital signals. If you do have parallel traces and are concerned with coupling to/from them, keep them spaces as far apart as possible.

    Distance to the ground plane similarly will not make a lot of difference at moderate frequency.

    If the signal has high frequency content, then it may be advisable to design the trace as a transmission line ("microstrip" if it is just over a ground plane, "strip line" if it is between two ground (at AC) planes). The width then is a function of the desired line impedance, the dielectric constant of the PCB substrate and the spacing between the trace and ground(s). You can find lots of info on the web about how to approach this. If you use a transmission line of necessity, then it also must be terminated in its characteristic impedance. For precision analog work it is typical to use series termination at the source end and parallel termination at the destination, but I doubt if you would require this.
     
  7. AnalogKid

    AAC Fanatic!

    Aug 1, 2013
    6,958
    1,971
    The external interference pickup will not be all that much, primarily because the output impedance of the IA will be near zero ohms, and 20 cm is 1/4 wavelength at around 200 MHz. Assuming whatever is receiving the signal is a relatively high impedance input, trace inductance will appear as an impedance that increases with frequency, making the system more susceptible to high frequency interference than low. You can further reduce susceptibility by placing a resistor across the differential pair close to the receiver input pins. This will load the IA output, so it is a tradeoff; a lower resistance improves noise performance but reduces the signal amplitude.

    ak
     
  8. DreeOlee

    Thread Starter New Member

    May 11, 2018
    3
    0
    Wow....this was my first post and thank you all for the reactions. I didn't expect this much reactions and knowledge on this Forum.

    The signals are low frequency around the 10kHz. In the construction it's not possible to add a cable, else a shielded twisted pair for differential signal or a coax for single line would do the job.
    As @ebp asked, I'm concerned about coupling into the signal from outside sources, EMS. I need the signal to be as clean as possible when it goes into the ADC.

    I've added 2 possible scenario's in the schematic underneath.
    Q1: Shall I transport a differential signal over 20cm or a single line signal over 20cm?

    As @DECELL suggested, keep the traces small and near by each other. I know this is a good EMI practice for high frequency digital differential signals.
    Q2: Is this also good for low frequency EMS?


    upload_2018-5-12_7-43-33.png
     
  9. crutschow

    Expert

    Mar 14, 2008
    19,363
    5,396
    To minimize pickup, keep the circuit impedance as low as possible.
    If you use the first circuit, R2 and R7 should be at the end of the traces, not the beginning.
    And reduce their value to a few kohm if possible.

    Depending upon the signal level, you could also amplify the signal, which reduces the relative amplitude of any interference voltage.
     
  10. ebp

    Well-Known Member

    Feb 8, 2018
    1,422
    477
    Although it may cost a little more, I would strongly recommend an integrated instrumentation amplifier instead of one made from individual op amps and discrete resistors. The performance of your circuit in terms of common mode rejection depends very greatly on the matching of the ratios of R2/R3 to R7/R8. In an integrated instrumentation amp those ratios are precision trimmed to much better matching and thermal tracking than you will get with discrete 1% tolerance resistors. If you don't have varying common mode at your inputs, then this is less of a concern, since errors in those resistors will translate to essentially fixed offset and gain error - which may still be important. Many integrated IAs have a reference input so you can conveniently use the reference you require.

    If you stay with your circuit, you might consider 0.1% 25 ppm/°C resistors, if you can obtain them. They are made by many companies and are usually not very expensive.

    With your circuit, I would say it is better to put the differential amplifier close to the input stage. If a signal were to couple into your differential pair from a circuit board trace running parallel to the differential pair, it would tend to couple more strongly to the nearest conductor and therefore not be rejected as common mode noise, This is why twisted pairs are used for differential signals - interference tends to couple more equally into both conductors.
     
  11. Picbuster

    Active Member

    Dec 2, 2013
    740
    90
    Use a multiple layer PCB and run this on the inner layer(s) however try to avoid long wires.
    It's not the produced radiation only buts also the received a twenty cm track will be an excellent antennae.
    The so received signal could also effect the other signals.
    The dc restore effect activated by the received signals could elevate or disturb input of the 10Khz receiver.

    Picbuster
     
  12. DreeOlee

    Thread Starter New Member

    May 11, 2018
    3
    0
    @crutschow and @ebp: thanks for the usefully tips!
    a multilayer PCB would really overkill this board, therefore I prefer to solve this case in a 2 layer PCB.

    For now I have an amplification of 9,33 and that is more than enough, else my signal will clip.

    I changed the circuit, my only question open is: should the differential trace be small or wide?


    upload_2018-5-14_9-25-16.png
     
  13. ebp

    Well-Known Member

    Feb 8, 2018
    1,422
    477
    Make them small (narrow) and close together. This will help a bit to make coupling from external sources equal in the two traces. The reality is that 20 cm isn't particularly long and not likely to cause any problems unless there is a nearby source of serious noise. At crutschow mentioned, it is too short to be a good antenna at lower frequencies.
     
  14. MrChips

    Moderator

    Oct 2, 2009
    16,503
    5,065
    If you are concerned about noise pickup on a very sensitive low voltage analog signal, my inclination would be to redesign the ADC interface.
    From instrumentation amplifier, differential input, differential output, drive differential input ADC with serial output (SPI or I2C).
    Then you can send the digital output across the 20cm.
     
  15. ronsoy2

    Member

    Sep 25, 2013
    61
    19
    It would help if you described the input signal levels and frequencies. If they are not really low level you may be able to randomly run the traces with no problem at all.
    If you are looking for ECG signal levels then you need to do a lot more consideration. (for sure put the gain in the input stage) If you are building an ECG amp the input op amp should be a low noise, low offset type such as a LT1002.
     
Loading...