Connect with us

Grounding

Discussion in 'Electronic Design' started by CeeRox, Aug 8, 2006.

Scroll to continue with content
  1. CeeRox

    CeeRox Guest

    Hi!

    Here a question that problably will have equal answers as there are
    engineers but I'll give it a shoot:
    Where is the best place to splitt digital and analog ground? For
    example, on a PCB there are both digital curcuits like FPGA or DSP and
    sensitiv analog ICs like sensors and op-amps. Beetween these digital
    and analog world there are ADCs and DACs. The most intuitive would be
    to split the ground at the different ADCs, but should this be done at a
    very narrow point and should the ground planes be seperated with a
    ferrite bead or just "0Ohm"..?

    /C
     
  2. Eeyore

    Eeyore Guest

    I use a slim track or a 'zero ohm' link.

    The important thing to consider is current flow. Ensure that 'digital currents'
    don't flow in the analogue ground.

    Graham
     
  3. colin

    colin Guest

    There are several ground methods wich people like to put forward as the
    'perfect' solution (ie solid aluminium ground chasis, star gnd,...) each one
    is good in its own way, but basically you need to consider the noisy
    currents from the digital supply grounds and make sure they dont cross
    through any part of the quiet ground plane so that they can introduce a
    voltage wich is added onto your quiet signal.

    However if you have multiple signals with multiple DACs, if they are all
    coming down the same shielded signal cable and on the same board then you
    just have one quiet gnd plane and one point at wich digital and quiet gnd
    are conected.

    I gues if you put conections with 0ohm you can always swap it for a ferrite
    bead, or even a 10ohm resistor.
    It realy all depends where the worst noise in the system is as to wether
    things like this make it better or worse.

    Oh and watch those supply decoupling caps too, dont forget they have most of
    the noisy currents through them.
    often the SPI interface introduces a more intrusive noise when it is sending
    bits, so it is worth making sure the currents in this path are contained.

    If you have seperate sources and seperate boards it gets more complicated as
    the current paths become more dificult to identify. It may be best to
    consider each one as seperate and not need to connect the quiet grounds
    together, however if their grounds are connected together at the far end (or
    at the case) a ground loop could arise wich acts like a loop antena.

    It is probably not practical to completly isolate the quiet grounds but a
    common mode torroid filter on the signal+gnd lead might help to get rid of
    induced circulating currents in the ground. A ferrite bead between the
    grounds might help to reduce this too, it might be best to connect the
    digital and quiet grounds together at just one place, but again wether this
    makes it better or worse depends on other things as the DACS might complain
    if there is a large signal between thier analogue and digital gnd.

    So suck it and see, or copy something similar that works well, or look at
    something that doesnt work very well and dont do it that way.

    Colin =^.^=
     
  4. Noway2

    Noway2 Guest

    Unfortunately, there is no one right answer to your question as it
    depends on the design and the situtation as there is no one definition
    of "Best".

    Both Dr. Howard Johson and Henry Ott have excellent web pages that deal
    with this subject. I would suggest checking them out.
     
  5. As others have indicated, controlling noise in circuits is a very
    large subject of which grounding is just one part. If you have a
    component or circuit that is particularly sensitive, running a
    separate ground and power traces from the power supply capacitors is
    probably the best strategy. With some of the new very low power
    microcontrollers, it is now possible to design boards that generate
    very little digital noise to begin with.
     
  6. John  Larkin

    John Larkin Guest


    Don't do it. Use a single solid ground plane and handle any low-level
    problems locally.

    Splitting planes implies an impedance between them, hence high
    relative AC potentials between "grounds". That will generally cause a
    lot more trouble than it cures.

    John
     
  7. Didi

    Didi Guest

    Don't do it. Use a single solid ground plane and handle any low-level
    Actually you can do it - and sometimes you must do it if you want your
    design to work.
    The best suggestion was already given by Graham,
    works for me as well.

    If you are doing just analog and digital, well, placement often (if not
    always) can be sufficient. However, if you have full scale input signal
    in the mV or tens of mV range, plus high speed sampling (1, 10 or
    more MSPS) at 14+ bits and, say, some smps on the same board
    which has to be small..... well, you have to split the ground plane -
    and
    some others as well.
    And again, there is no better advice which can be given than the
    one Graham already gave - if it is not detailed enough for you, you
    need to gain more experience/knowledge rather than an advice.

    Dimiter
     
  8. Joerg

    Joerg Guest

    Hello Dimiter,


    I'll second John's comment. In 20+ years I have yet to see a split
    ground situation that performed well enough. Except where safety
    concerns or regs mandate a complete isolation, there we just had to make
    it work.
    It hasn't for my clients.


    On the ultrasound systems we designed the signals range from almost down
    in the thermal noise to tens of mV. Works fine with a solid common
    ground plane but didn't with splits under the ADCs.

    OTOH I won't complain about designs where people have split the ground
    plane. After all, that brings in re-design business for me :)
     
  9. Eeyore

    Eeyore Guest

    Not in the case of audio. You have to be careful where those ground currents
    flow.

    Graham
     
  10. Eeyore

    Eeyore Guest

    Many reference designs use 'split' grounds.

    There's a bit of a clue when the chip itself has dedicated AGND and DGND pins !

    Graham
     
  11. Didi

    Didi Guest

    Hello Joerg,
    how many bits conversion? Do you have an SMPS on the same
    board (tiny enough - like 100 x 50 mm ).
    Well like I said it works for me. Check my hi-spec gamma spectrometry
    module for an example.
    Well then give it a shot at my competitors. A number of them would be
    glad to match my above mentioned module - they all have yet to do so
    four or five years after I introduced it.
    I'll be "gespannt" . :)

    Dimiter
     
  12. Eeyore

    Eeyore Guest

    I think it's a case of horses for courses. I did actually once try a non-split ground
    for a DSP processor in some audio gear I was designing for the heck of it and the
    digital section introduced 'birdies' into the audio at low level. Back to plan A !

    Graham
     
  13. Keith

    Keith Guest

    Not always. Several of our chips have separate AGND and GND pins,
    but the intention is *not* to go to different grounds. It's to
    isolate the on-chip digital noise from the PLL. It's the package
    inductance along with huge switching currents that's the problem,
    not card plane noise.
     
  14. Joerg

    Joerg Guest

    Hello Dimiter,

    12 bits at over 100MSPS. Plus a time-gain control amp in front to cover
    the required range.

    Yes. But the boards are typically larger, about pizza size. Except one
    that was a litte under 100mm x 150mm. Size didn't really make a
    difference. However, this stuff has to perform under heavy duty RF loads
    such as a nearby diathermia machine. The worst case would be a
    defibrillator shock while the patient is still connected. That's not
    supposed to happen but cardiologists can make mistakes after a week of
    hard overtime and lack of sleep.
    I've never worked in that field. I like the bus designator "Nukebus" on
    your web site.
    I wouldn't know who your competitors are but you can give them my web
    site address ;-)
     
  15. Eeyore

    Eeyore Guest

    Sounds like you're working at somewhat higher freqiencies than me ! ;~)

    Graham
     
  16. Joerg

    Joerg Guest

    Hello Graham,
    Very low frequencies is where star-grounds and stuff like that can
    indeed work. Ultrasound guys consider audio to be DC ;-)

    Problems can still creep up when you install such split ground gear in
    the vicinity of a strong RF emitter. Radar bases, coast guard stations,
    AM talk radio towers, 13.56MHz "blasters", you name it, I have seen them
    pretty much all. Mostly I have to come out there to find out what's
    causing EMI and then sit down with the client to gently break the news
    that they need a few re-layouts and chassis mods. Usually the engineers
    take that in strides but often the enclosure designers don't. Frequently
    they are artists rather than engineers and they can become quite livid
    when I suggest to move away from an injection molding scheme.
     
  17. John Larkin

    John Larkin Guest


    Just recently, I put a power supply (linear and switching regs), a
    temperature controller (thermocouple-input, 150 watt PWM heater
    output), a PPM-noise-level, 3-amp NMR gradient coil driver, and a uP
    on a single small board, with a single ground plane. Works fine and
    passed FCC and CE first time.

    And another board has a VME interface, switching regs, uP, and twelve
    12-bit ADCs clocked at 40 MHz, with sub-LSB RMS noise levels. Single
    plane.

    I also did the NIF timing system: about 2000 client points triggered
    to within a few picoseconds accuracy, spread over the world's biggest
    laser, the size of a football stadium. No split planes there, either.

    And how about these?

    http://www.highlandtechnology.com/Pages/prodind2.html

    Not a single split plane in the bunch.


    Is that enough experience?

    John
     
  18. Jim Thompson

    Jim Thompson Guest

    Crap. Graham can't even give good advice on how to wipe ;-)
    Yep. You don't want a common wirebond to cross-couple noise.

    Very standard practice in the microchip world.

    ...Jim Thompson
     
  19. Guest

    The answer is pretty straight forward once you figure out if you
    dealing with high level digital current, low level digital currents,
    single or multiple boards, see

    http://www.analog.com/en/content/0,2886,760%5F%5F97529,00.html
     
  20. Joerg

    Joerg Guest

    Hello Graham,
    Plus professors often teach that stuff. That, and those reference
    designs, have kept my business humming. When I started out I really
    didn't want to go into EMI but split grounds have kind of sucked me into
    that funnel.

    It can also mean that the chip designers didn't have much of a clue
    about the system side of things ;-)

    The worst case was a slew of field failures. Some pulses had hit into
    the substrate diodes and much of the stuff across the AGND-DGND devide
    fried. Nobody knew where the pulses came from but after a re-layout with
    a common plane there were no more field failures.

    In EMI we have an old rule: The EMI performance of a given design is
    inversely related to the number of toroids it requires to make it behave.
     
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

-