1. This forum section is a read-only archive which contains old newsgroup posts. If you wish to post a query, please do so in one of our main forum sections (here). This way you will get a faster, better response from the members on Motherboard Point.

Analog and digital GND

Discussion in 'Embedded' started by Frida, Jan 27, 2005.

  1. Frida

    Frida Guest

    Hi, I am using an ADC with 8 single ended inputs, and for a referensvoltage
    I have a REF02. In the datasheet for the ADC it is quite specified how the
    GND-pins should be connected (to AGND), but how about the decoupling
    capacitanses on the inputs. First I have 2 decoupling capacitanses on the
    VCC-input and then I have 2 on the Vref-pin. But are they suppose to be
    connected to AGND or GND. My intention is to have 2 separate ground-planes
    at the same potential (0V) and then just connect them in one single point,
    also here decoupled. So I have the REF02-circuit connected to AGND and the
    ADC, but how should I do about the capacitanses in the inputs?? should
    they be connected to GND or AGND??

    Thank you!!
    Frida, Jan 27, 2005
    1. Advertisements

  2. Further reading in an application note reveals that the ADC
    is supposed be mounter on the AGND with its AGND and DGND
    pins on the AGND. Go ahead, there are quite extensive
    application notes at the various manufacturers websites.

    Rene Tschaggelar, Jan 27, 2005
    1. Advertisements

  3. Frida

    Frida Guest


    I am sorry if I wasn't clear. You are absolutely right, the datasheets
    specify clearly how the pins on the ADC should be connected. But it
    doesn't say anything about the decoupling capacitances. So my questiod was
    really about them and not really about the ADC itself. Should the
    decoupling capacitances be connected to AGND or GND?? Or maybe is it
    implicitly saying that the decoupling capacitances should be connected to
    the same ground as the ADC, but that is what I can't find out.

    Thank you!
    Frida, Jan 27, 2005
  4. Use a unique, large, full ground plane, and connect all pins that should be
    connected to all xGND to this ground plane. This is by far the safer
    alternative for 99,999% of the designs. Dual-ground plane architectures are
    VERY difficult to design, and are the root cause of serious headackes when
    doing EMC testing... Except of isolated / high voltage designs of course.

    Anybody disagree ? (this is a subject discussed quite often so I expect
    thousands of answers ranging from "stupid answer" to "of course"....)

    Robert Lacoste, Jan 27, 2005
  5. Frida

    CBFalconer Guest

    To GND. The underlying principle is that there should be no
    currents flowing in the AGND circuit. Currents have spikes, and
    cause IR drops, and generally create havoc for analog inputs.
    Decoupling capacitors shunt current in order to maintain voltages.
    CBFalconer, Jan 27, 2005
  6. Frida

    Guy Macon Guest

    The answers will be far more likely to be correct if the question
    is asked in sci.electronics.design where it is on-topic. While it
    is true that some EEs are also interested in embedded systems
    programming, many are not and thus don't read comp.arch.embedded.
    Guy Macon, Jan 27, 2005
  7. Frida

    Joerg Guest

    Hello Robert, Hello Frida,
    Amen. Meaning I agree and thus I guess I'll fall into the category "of
    course". In my 20 years on the beat I have never seen a split ground
    system work well. A few of them kind of worked but then they didn't pass
    EMI until we performed a common ground relayout.

    One way to think about it is that a typical system has more than one
    connection to the world. So while there may be just that single ground
    connection under the ADC there are signals coming in from the analog
    side to be converted and then other signals going to displays, keyboards
    etc. on the digital side. All these will also carry ground leads. This
    causes lots of not well controlled loops with each of them having to be
    broken by ferrites or other means, something that rarely works well.
    This is just one of the reasons why a split ground architecture can lead
    to sleepless nights.

    On my designs I always start out with a nice full ground plane and make
    sure that any currents on that plane won't cause more transients at the
    converter than can be tolerated. It has never been a problem, as long as
    the placement of components is suitable.

    Cordialement & med bästa hälsningar, Joerg

    Joerg, Jan 27, 2005
  8. Frida

    Tauno Voipio Guest

    It's there - between the lines: if the only ground connected
    to the chip is AGND, the by-pass capacitors have to be connected
    to it.

    A different story is that the incoming power supply
    should be decoupled by a choke to avoid polluting
    the analog ground with the crud on the supply line
    via the caps.
    Tauno Voipio, Jan 27, 2005
  9. Depends on what is meant by 'split ground'.

    I regularly use a star ground that is then grounded to the 'system' ground
    at the center of the star. This creates a 'ground plane', though a
    pretty cruddy one as the lines going to the star are not gridded.
    Often more than one star.

    And I have had boards that were split horizontally - left half of
    the board analog and right half digital. 5v and Dground layers for the
    digital side and +/- V and Aground layers on the analog side.
    One connection between the two grounds made at the power-supply
    reference point.

    For process control instrumentation it is not uncommon to have one
    ground per process input/output. The back panel of process control
    cabinets often have a drilled copper bar for _the_ signal ground
    (used to be labeled 'Mecca Ground'). Often sensors are grounded at
    the source.

    I haven't had any problems with the exception of clients who insist
    on 2-layer boards for high speed designs. The problem has been
    EMI susceptibility.

    Nicholas O. Lindan, Jan 27, 2005
  10. Frida

    Joerg Guest

    Hi Nicholas,
    EMI is usually the first problem I find with approaches that didn't use
    a single gound plane. It was more prevalent than performance issues
    (although there were tons of these, too). A split or otherwise separated
    plane makes for a nice big dipole antenna that radiates and receives.
    Any RF currents flowing across the node where they are connected are at
    the same time imposed onto that unwanted dipole antenna. Inevitably any
    system will have some physical connections to the rest to the world.
    Then these dipoles become huge loop antennas and it all gets even worse.
    Just my experience, and I have seen it over and over again.
    Until now I or rather my clients haven't gotten any mileage out of
    separate ground approaches, except the miles for the repeat trip to the
    EMC lab ... ;-)

    Then again, many EMC labs are located in rather pristine areas of the
    country so everything has an upside.

    Regards, Joerg

    Joerg, Jan 27, 2005
  11. Fully in agreement with Joerg. In fact in you use a "split" ground plane
    with a unique connection under an ADC chip, then in order to avoid any
    EMI-receiving/emitting coil you have only one solution : All signal lines
    going from one side to the other must be routed EXACTLY ABOVE the connexion
    point between the two grounds ! If not you have a marvelous current loop...

    Robert Lacoste, Jan 28, 2005
  12. Frida

    Joerg Guest

    Hello Robert,
    Yes, and when the product is now behind schedule the only way to fix
    these loops is with the 'Aspirin method'. Lots of #43 material toroids
    and other cores. The worst case I ever saw required about two pounds (!)
    of ferrite to make it perform and pass EMC. Later after a redesign with
    a common ground structure that dropped to zero pounds, with even better
    EMC margins. The only sad person was the sales guy of the ferrite supplier.

    Regards, Joerg

    Joerg, Jan 28, 2005
  13. Frida

    joep Guest

    techonline has a good analog lecture on A/D grounding you may want to
    joep, Jan 28, 2005
  14. Frida

    Johnny Guest

    The VCC supply is for the digital circuitry of the ADC chip. It will
    therefore be noisy, so the decoupling capacitor should be connected to
    digital groud.

    The suggestion of having only one xGND plane will obviously work, and
    is a good solutions for many applicaitons if you have a very solid
    ground plane and are not critically concerened with ADC accuracy.
    However, if you need to measure very small signals or get ultimate
    accuracy, then you need to have separate AGND and GND planes that are
    connected at only at a single point.

    Johnny, Jan 29, 2005
  15. Frida

    joep Guest

    I think the folks here (as well as the a/d manufacturers) are
    suggesting a single ground plane is the best solution (lowest noise)
    not a comprimise solution for the majority of cases when using
    commerical A/D's. I think the reason is that an A/D is already an
    integrated mixed signal device and you have to deal with the
    complications and limitations of the grounding system thats brings.
    Connecting its GND to a seperate GND plane(assumed noiser) can
    internally couple noise into the analog portion of the a/d via stray
    capacitance. For the rest of digital circuitry on the board the idea is
    to physically seperate them from the analog devices on the board so
    that the returns of the noisy digital chips don't have to cross over
    analog returns to get back to the power supply return.

    Obviously there are exceptions to this rule especially for strange
    shaped PCB's or motherboard/daughterboard designs, or discete optically
    isolated A/D's but for large single pcb systems using integrated A/D's
    or microcontrollers, its a pretty reliable option.
    joep, Jan 29, 2005
    1. Advertisements

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.