Connect with us

Analog/Digital supply / ground ?

Discussion in 'Electronic Design' started by Sylvain Munaut, Apr 12, 2004.

Scroll to continue with content
  1. Hello,

    I have a small design question :

    Components that interface to the external world like USB, firewire,
    video encoder, ... have the notion of Analog Ground & Analog power. Is
    is ok, if I connect them to the digital ones at a point that is near the
    component that needs them and not close to the power supply, but I would
    connect them trhu a :

    Main VCC ----(_)(_?µH_)(_)----|---- Analog VCC
    --- ? µF

    Main GND ----(_)(_?µH_)(_)------ Analog GND

    Would that be OK ? And what values to use for the inductors ?

    Sylvain Munaut
  2. Joerg

    Joerg Guest

    Bonsoir Sylvain,

    in most cases I found that connecting all ground pins to a common ground
    plane via the shortest possible path works best. As long as that is a nice
    plane over the whole circuit board. I had to redesign many, many systems to
    that common ground scheme because they were very noisy and wouldn't pass EMC
    tests otherwise.

    As to supplies, these can be separate but must have bypass capacitors to the
    ground plane very close to the supply pins. Also, sometimes the power has to
    come up in a prescribed sequence but that would be found in the data sheets.

    Connecting the rails from two different power supplies via an inductor is
    something that should never be done. If one comes up later or for some
    reason not at all this could result in a nice fireworks.

    A bientot,

  3. Bonsoir également ;)
    Thanks for the answer.
    Yes, I have a complete ground layer. So just leaving it as plain as
    possible will do even for mixed signals, cool ! That of course simpler.

    I only have one supply by voltages. And all the voltages are
    monitored/tracked so that poweron/poweroff sequence are with a common
    rising/falling ramp. It also have 'emergency' shutdown of all voltages
    if for any reason one of them wouldn't come up.

    I have many voltages & many components requires some sequencing so I
    took a great look at that. I have 12V, 5V, 3.3V, 2.5V, 1.5V, 1.2V, -5V.

    Wow, that not what I meant. It's just that I only have one power supply
    that provides for example 5V and that I need it for digital Vcc and
    Analog Vcc.
    So I'd use a Inductor & Capacitor to prevent the noise generated by one
    to go to another.

    Sylvain Munaut
  4. Joerg

    Joerg Guest

    Hi Sylvain,

    Yes, breaking up the 5V can make sense. Run it directly from the 5V plane to all
    digital pins and then a small RC or LC filter to very sensitive analog pins, with
    the capacitor very close to the pin.

    Then everything should be "tres bien". That's about all the French I know, wish I
    knew it better. But out here in California we have to learn Spanish more than
    French because we so close to Mexiko.

    Au revoir,

  5. Thanks, how can I estimate the values of the L & C.
    Also, for the Capacitor, there is multiples 'types' and I'm sometimes
    lost ...

    ;) Here there is no problem, we learn English. And even more in
    electronics/computer world.

    Was it that obvious that I'm french ?

    Sylvain Munaut
  6. I read in that Sylvain Munaut <>
    Not from what you wrote; it's perfectly normal English. Well done!
  7. Paul Mathews

    Paul Mathews Guest

    Inductors: There is a tradeoff among these factors - Size and cost, DC
    resistance, B-field emissions, and saturation current. Also, some
    types of inductors are deliberately lossy. Anyway, it takes some
    study to choose the best type for an application. In general, choose
    the highest inductance that will fit in available space at an
    allowable cost that also has acceptably low DC resistance and
    sufficient saturation current.

    Capacitors: Multi-layer ceramic capacitors usually provide the highest
    performance. With all capacitors, effective series resistance and
    inductance limit performance at high frequencies. Impedance rises
    beyond the self-resonant frequency, as seen on detailed datasheets,
    Chip ceramic capacitors in wide packages have the highest
    self-resonant frequencies. Choose the capacitor(s) with the lowest
    impedance at the highest frequency of interest.

    Hybrid filters: TDK, Murata, and Panasonic (possibly others) offer
    excellent hybrid LC filters. These are your best bet if you remain

    Paul Mathews
  8. Joerg

    Joerg Guest

    Hi Sylvain,

    Usually it is best to use SMT ceramic caps. 0.1uF is popular and when you expect very
    high frequency noise maybe a 0.01uF in parallel, and the smaller one closest to the

    If it draws only a few mA then I often opt for a 5 to 10 ohm resistor. Make sure you
    don't cause problems with it's voltage drop. For an AD converter, for example, this
    resistive filtering may not be a good idea. Otherwise a small wire and ferrite bead is
    a good option. Place a drop of glue on the bead to avoid that nasty rattling noise.
    These kind of "bead chokes" also come in SMT, check Panasonic and the other inductor

    As John said, your English is perfect. But your name sounds French and the way you
    spelled your location does. The Flamish speaking folks in Belgium would have called it
    "Leuven" I believe. I used to live not far away in the tiny village of
    Vaals/Netherlands. There I spent a lot of time with Belgian racing bike riders of both
    languages. Oh, do I miss that Belgian beer...

    Greetings, Joerg.
  9. I read in that Joerg <[email protected]
    SMT caps have very little inductance, so it is often optimal to have a
    30:1 ratio, i.e. 100 nF and 3.3 nF.
  10. Thanks a lot for all theses advices.

    Sylvain Munaut
  11. Hi
    Thanks, I think I'll put single 100nF SMT ceramic cap for each
    non-critical chips, 100nF & 3.3nF near each high-frequency chips and use
    an LC filter for all chips that need a such called "Analog supply".

    Actually there is two city :
    - Louvain La Neuve ( where I am, mainly a 'university campus city' )
    - Louvain ( AKA Leuven for the Flamishs ) that is not far away but
    it's a classic city.
    Sure that I do appreciate some good special beers too.

    Sylvain Munaut
  12. Ok, thanks. Just out of curiosity, where does that 30:1 ratio comes from ?

    Sylvain Munaut
  13. I read in that Sylvain Munaut <tnt_at_246tNt_dot_
    You look at the impedance/frequency curves of the caps, which most
    manufacturers provide now, and see which parallel combinations give you
    the lowest impedance over the largest bandwidth.

    Two caps in parallel create a *parallel* resonance (roughly, the smaller
    capacitance with the inductance of the larger one). A large ratio of
    capacitances tends to minimise the bad effects of this resonance.
  14. Rich Grise

    Rich Grise Guest

    I've seen mixed circuits - specifically 16-bit DACs - with two separate
    planes on the same PCB, connected together at the ground pin of the edge
    connector. Or maybe it was at the ground pin of the DAC itself. The Burr-
    Brown guy could probably say which is better.

    Good Luck!
  15. Joerg

    Joerg Guest

    Hi Rich,

    Dealing with these situations is my bread and butter. Many data books and
    university courses advocate split grounds. But I can't recall one case where
    that has worked reliably on a complicated mixed signal board. I always ended up
    recommending a relayout with one single plane and things became really quiet.
    Not that I would say that this is generally the case, I just haven't seen split
    ground work too well.

    Regards, Joerg.
  16. Beau Schwabe

    Beau Schwabe Guest

    In IC layout the reason for having separate grounds is to help reduce
    noise. In Example 1 suppose that ckt GND #1 is supplying power
    to something very current hungry making lots of noise. Because of
    the IRD (Current vs. Resistance Drop) this noise becomes exaggerated
    and will flow into ckt GND #2 more readily. If you look at Example 2,
    you will still notice IRD, but because you have two separate lines to
    supply GND current the "bleeding" from one circuit to the other is
    greatly reduced.

    Suppose you have a circuit....

    Example 1:

    IRD #1 IRD #2
    GND source >----/\/\----o----/\/\----> ckt GND #2
    o--> ckt GND #1

    Example 2:

    IRD #1
    o---/\/\----> ckt GND #1
    GND source>-o
    | IRD #2
    o---/\/\----> ckt GND #2
  17. KR Williams

    KR Williams Guest

    I've done it successfully. Indeed one design (years ago) I
    deleted the planes under the analog input section since the
    capacitance of the signal to ground (back to signal) was too
    high. The layout people thought I was nuts, and the wires going
    nowhere (driven guards) helped their case. ;-) It worked better
    than expected first time out, which helped my case. ;-) To be
    fair, the layout people were used to "high frequency" logic
  18. John Larkin

    John Larkin Guest

    I've never understood why anybody would waste a board layer just to
    create two grounds that are at *different* potentials. The IC
    manufacturers think their part is the center of the universe, so ask
    us to connect the planes at their (presumably single) chip; this is
    silly. (The university professors think *they* are the center of the

  19. Roger Gt

    Roger Gt Guest

    X-No-Archive: yes
    "John Larkin" wrote
    : Joerg wrote
    : > Hi Rich,
    : > Dealing with these situations is my bread and butter.
    : > Many data books and university courses advocate split grounds.
    : I've never understood why anybody would waste a board layer just
    : create two grounds that are at *different* potentials. The IC
    : manufacturers think their part is the center of the universe, so
    : us to connect the planes at their (presumably single) chip; this
    : silly. (The university professors think *they* are the center of
    : universe.) John

    Not necessarily "TWO" layers, just isolated on the same layer. I
    have used as many as four with the final (Mecca) connection at the
    input power connection (8 pins) so all parts of the board had the
    "SAME" potential rather than one circuit raising or inserting
    noise into another circuit which needed a lower level of ground or
    noise on the ground. Sometimes just the power bypasses are
    contributors to a noise level if the clock rates are high and not
    all the grounds are low enough impedance.

    Guard lines are particularly good with very high frequency and
    high impedance circuits to maintain a constant reference to a
    non-conducting ground level.

    Roger Gt.
  20. EEng

    EEng Guest

    Rather than a solid plane I use grid planes, like a printed faraday
    shield. I keep analog and digital grounded together, and if there's
    audio or rf, their planes are connected to the others via a 47uH to
    100uH inductor. Its still one ground, but with some control. Never a
    problem, although once there was a serious 60Hz hum due to power AC
    on the board, but that was fixed with an inline filter.
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