Connect with us

ground question

Discussion in 'Electronic Design' started by j.f.deleon, Jan 10, 2004.

Scroll to continue with content
  1. j.f.deleon

    j.f.deleon Guest

    If in a device I have sub circuit-A (sensitive input circuit) and sub
    circuit-B (power output circuit), common sense dictates that power
    supply and ground return should be different for each sub circuit.
    The question that I would like to ask the group is how much of a
    current difference should exist between circuits A and B before a
    designer considers a separate supply and ground return. I would
    appreciate any rules of thumb or computation that you guys can pass my
    way. I am particularly interested in guidelines for discrete analog
    (Please note that I am only into hobby electronics so please go easy
    on the math if any).

    Thanks very much,

  2. mike

    mike Guest

    Since you didn't give any numbers, math would be useless.
    (There I go again inviting argument. Arithmetic would be useless.
    Surely, math could be used)
    You usually want a star ground from each stage to the power supply.
    You usually (I started out with ALWAYS, but that would have just
    started an argument) want a linear ground that follows the signal path.
    Hmmm, conflict! You make tradeoffs depending on the specific
    characteristics of the application. If you can't make it work single
    ended, a differential signal path goes a long way to resolve this conflict.
    So, it depends on how sensitive? current difference where? frequencies
    involved? In a word...specificity!

    Return address is VALID.
    Bunch of stuff For Sale and Wanted at the link below.
    Toshiba & Compaq LiIon Batteries, Test Equipment
    Honda CB-125S $800 in PDX
    TEK Sampling Sweep Plugin and RM564
    Tek 2465 $800, ham radio, 30pS pulser
    Tektronix Concept Books, spot welding head...
  3. I read in that j.f.deleon <>
    It's not directly related to the 'current difference'. The principle is
    that *supply and return conductors should not be shared between circuit
    functions*. This is true even for, as an example, the avoidance of
    crosstalk between the two channels of a stereo preamplifier, where the
    'current difference' is zero (current ratio of 1).

    A second issue concerns electrical 'noise' on the supply conductors. If
    a circuit imposes noise, it should preferably be filtered at source,
    using shunt capacitance and, if necessary and practicable, series
    resistance and/or inductance. If it is not sufficient to filter at
    source, that the supply/ies to sensitive circuits need to be filtered,
    using the same types of component, shunt capacitors and series resistors
    or inductors, or perhaps voltage regulators if the noise extends to very
    low frequencies and the sensitive circuits can operate with reduced
    supply voltages.
  4. CFoley1064

    CFoley1064 Guest

    If in a device I have sub circuit-A (sensitive input circuit) and sub
    Go to a beach, expect sand; go to a design forum, expect a technical answer. I
    guess the best non-math, non-technical way to express it is to say that your
    grounding scheme has to be good enough so that ground loop problems don't
    interfere with what you need from your circuit.

    Ohm's Law (V = I * R) is how you calculate voltage drops across traces. The
    voltage drop across a trace is equal to the current times the impedance.

    A good primer on grounding issues with minimal math is the Analog Devices app
    note AN-202, An IC Amplifier User’s Guide to Decoupling, Grounding, and
    Making Things Go Right for a Change By Paul Brokaw

    It's well worth the time spent to read (8 pages), and will at least give you
    some understanding of what's going on.

    While you're in the neighborhood, you might want to browse through some of
    their other app notes:

    Good luck
  5. James Meyer

    James Meyer Guest

    Common sense does not dictate anything of the sort.

    Common sense does tell us that due to currents in ground elements,
    traces, or wires, and the fact that there are always unavoidable resistances
    involved with those elements, that careful analysis of the physical layout of
    the circuits needs to be done to make sure that any voltages developed from one
    end of a ground element with respect to the other end don't add unwanted
    voltages to signals that are referenced to the opposite ends of the ground

    In other words, the schematic of a circuit is not the circuit and you
    can't just place a ground symbol somewhere and expect that grounded point to be
    at the same potential as all the other ground symbols in the system.

    Even if you did use two power supplies, one for each sub circuit, you
    still have the problem of connecting the signals between subsections. Unless
    you use transformers or opto isolators, there will have to be a connection
    between grounds somewhere.

    Each and every design needs to be considered on its own merits. There
    are no universal rules of thumb that you can adopt and implement that will
    always result in a good design.

    Most designers can look at a schematic or system design and get an
    intuitive feel for what voltages will be present at each node. Fewer designers
    can look at a schematic and get the same feel for the currents involved. Fewer
    still can estimate what happens to those currents when the ideal ground symbols
    of the schematic are replaced with real circuit traces, ground planes, and

  6. Mac

    Mac Guest

    One approach to grounding is to use a ground and power plane on the
    circuit board. Then apply adequate distributed decoupling capacitors to
    the board. Then make sure each noisy IC has a good decoupling cap near it.

    If the circuit is all digital or all analog and the power is not too high,
    this will probably be good enough. (If it is all digital this WILL be good

    Things that need special treatment are switchmode voltage regulators and
    digital clock sources, as they are infamous for putting noise on a board.
    With switchmode regulators, most people realize that the output needs a good
    filter, but the input should be LC filtered, too, since it will pull current
    in a large square-wave otherwise.

    Keep other signals away from crystal oscillators and clock
    buffers/drivers, and put plenty of decoupling caps as close as possible.

    I've never had to mix high gain analog amplifiers together with high-speed
    digital circuitry. I imagine that this would be very challenging to get

    Anyway, if the ground is a little noisy with respect to Earth ground, this
    is not the end of the world provided that the inputs are differential, and
    provided that there is plenty of decoupling between ground and power.

    Just my $0.02.

  7. mike

    mike Guest


    What's the current thinking on ground plane resonances?
    'bout 20 years ago I was building a computer board with power/ground
    planes. I stuck a sweep generator into vcc/ground planes on one
    end of a bare board and looked what came out on the other side of the
    board. There was a broad resonance, a dip in the frequency response
    in the 10's of MHz. range. Then I started installing 0.1uF 1206 bypass
    caps. The resonance got sharper as I added caps, but the frequency
    stayed about the same. So, there was very low impedance at the resonant
    frequency of the system. The more caps I added, the higher the impedance
    got off resonance as the Q increased.
    The board worked, so I didn't pursue it further, but I'm still curious
    about how one would design a board with uniformly low impedance between
    VCC and GND planes. Or maybe the effect I was measuring is irrelevant?

    Return address is VALID.
    Bunch of stuff For Sale and Wanted at the link below.
    Toshiba & Compaq LiIon Batteries, Test Equipment
    Honda CB-125S $800 in PDX
    TEK Sampling Sweep Plugin and RM564
    Tek 2465 $800, ham radio, 30pS pulser
    Tektronix Concept Books, spot welding head...
  8. To expand on what others said:

    Current in the supply and ground traces, times the resistance of the traces,
    causes voltage fluctuation.

    For a given subcircuit, you can calculate its sensitivity to fluctuations:
    for instance, an amp stage might have no rejection of ground ripple (meaning
    that its output is ground-referenced, that is, any ripple on its ground
    shows up on its output) but 60dB rejection of supply ripple (meaning that 1V
    of ripple on the supply line will produce 1mV of ripple on its output).

    Then it's a matter of knowing how much interference you can tolerate. (The
    interference will show up either as noise, if the ripple is uncorrelated to
    the signal, or as harmonic distortion if it is correlated - for instance, a
    push-pull output stage causes rectified half-wave current on the supply
    lines, which looks like even harmonic distortion when it couples back into
    the signal.) If you can only tolerate 1uV of junk on the output, and you've
    got 60dB rejection of supply junk, then you'd better have 1mV or less junk
    on the supply. If the supply trace has a resistance of 0.1 ohms, you'd
    better have less than 10mA of junk current going through it (0.1 ohms times
    10mA = 1mV). And that in turn puts a constraint on what the supply trace
    can be shared with.
  9. Mac

    Mac Guest

    About two months ago, I attended a UL sponsored one-day seminar on EMC/EMI
    issues. They said that in theory (simulation) a circuit board could
    resonate a bit like a transmission line. But no one had ever heard of it
    actually happening or causing an EMI problem.

    Maybe the devices between the power planes provide way too much damping
    to allow any oscillation. Anyway, it doesn't seem to be a problem in

  10. Tim Shoppa

    Tim Shoppa Guest

    I think that you are implying that something in the PCB layout was
    responsible for the resonances, sort-of like a waveguide.

    For a 30MHz resonance, this implies a wavelength of 10 meters. Just how
    big was your PC board? :) It seems more likely to me to be the result
    of the passives on your board than the board itself.

    If you were asking about the 10GHz region, I do know that microwave engineers
    do have to treat PC board layout as waveguides for those high frequencies.

  11. I read in that Tim Shoppa <[email protected]> wrote (in <>)
    about 'ground question', on Fri, 16 Jan 2004:

    [snip: with trepidation. I may have snipped something crucial.)
    Given the permittivity of FR4 being about 4.7, AIUI, and the likely
    contribution of passives to both inductance (100 nF caps at 30 MHz) and
    capacitance (smaller caps, below self-resonance), it doesn't seem to me
    to be very unlikely that a resonance effect could be observed.

    Woodgate's Corollary to Murphy's Law states that 'Anything that can't go
    wrong, actually can.'. So if there is a fleeting chance of resonance,
    someone will experience it.
    Indeed, but that is fairly obvious.
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day