Connect with us

Doubt about decoupling capacitors in high-freq PCBs

Discussion in 'Electronic Basics' started by Mayank Kaushik, Feb 21, 2005.

Scroll to continue with content
  1. Hi,

    Im a total newbie to PCB design, i have to build a high-speed PCB for a
    board containing an Atmel At91 microcontroller operating at 200MHz,
    with RAM, Flash, etc, so im trying to collect info on PCB design.

    The question may be a bit misleading, heres the actual dope:
    Ive seen high-speed PCBs where not all of the decoupling capacitors are
    included on the final board, even though the schematic may mention all
    of them.How does one decide which decoupling caps can be safely omitted
    in the final design?

    Also, in an earlier design using the same controller as above, we had
    the RAM and the controller on seperate boards, connedted with a 20cm
    long ribbon cable. But the RAM wasnt functioning correctly, we were
    getting garbled data when we tried to store stuff on the RAM..could it
    be due to the fact that the RAM and the uC were on seperate boards??


    Thanks in anticipation,
    Mayank
     
  2. Bob

    Bob Guest

    Mayank,

    Determining if you've omitted too many capacitors is a difficult question.
    The easiest way to tell is to hook up a high-speed scope (with a
    differential probe) to the power supply (right at the chip pins or balls).
    Then, see if the supply ever dips below its rated limits.

    As far as the faulty RAM (with the longer cable), there are (at least) two
    possibilities:

    1) The setup time required by the RAM or its controller has been violated
    due to the longer transit time.
    2) The clock line, to the RAM, has not been terminated properly. So, the
    clock edges (at the RAM) may not be monotonic.
    3) There may be crosstalk, in the cable, causing the clock edges (at the
    RAM) to be non-monotonic.

    #2 or #3 are the more likely candidates, but it's hard to tell without
    taking measurements on your setup.

    Bob
     
  3. John Larkin

    John Larkin Guest

    It's common, nearly universal, to design in too many bypass caps; I've
    seen boards with hundreds and heard of boards with thousands. Most
    people just leave them in, but one can measure rail noise and remove
    caps to cut cost.

    I know a guy who does dense digital boards and doesn't use bypass caps
    at all. Personally, I've never done a board that had too few, so he
    may be right.
    Unless everything was properly terminated, and the critical sigs were
    straddled by grounds in the cable, and the prop delays were
    calculated, and there are no ground loops, this can be very bad news.

    John
     
  4. "John Larkin" <>
    wrote in message ....

    I once designed a MultiBus card with its area divided into
    about 1/3 ECL, 1/2 74Fxx TTL, and some analog stuff.
    The logic was running near the upper edge of its frequency
    range, (some of the time). Much of the logic was stateful
    and several different clocks traveled across the board.

    According to my calculations, the digital sections needed
    a total of about 11 bypass capacitors if well placed. The
    board was layed out to meet my placement criteria. While
    verifying prototypes, I performed the procedure you just
    mentioned. What surprised me was that not only could I
    remove all the bypasses, but I could not observe any real
    increase in the rail noise after doing so.

    Since then, I have been a great fan of adjacent power and
    ground planes for digital circuits. Most logic (excepting
    ECL) is equally hard on both rails.
     
  5. John Larkin

    John Larkin Guest


    If you do a multilayer board with a thin dielectric between the ground
    plane and power planes (or even power islands) it doesn't matter much
    where you put the caps; the planes themselves are a superb capacitor.
    I sometimes add a few SMA connector footprints to a board layout so I
    can TDR the planes. As near as my Tek 20 GHz TDR can tell, a typical
    power/ground plane pair looks like an ideal capacitor, and adding
    bypasses anywhere just makes it look like a bigger ideal capacitor.

    And this stuff about microstrip return current getting confused when
    "the reference plane changes" is 99.44% nonsense. Some people are
    obscessed with this silly return current idea.

    If chips can change Icc grossly, like a CPU sleeping and getting an
    interrupt or something, you do need something to supply the gross
    energy without drooping too much.

    John
     
  6. Rick

    Rick Guest

    If you do a multilayer board with a thin dielectric between the ground
    But isn't the point of decoupling CAPs twofold - to stabilize the energy
    source and to shunt higher frequency signals to ground ? Wouldn't having
    only a large capacitance value from the physically large power and ground
    planes be counter productive to that ?
     
  7. [Apparently quoting John Larkin]
    But the point is, the high frequencies need not reach
    the larger discrete capacitances. They are shunted
    thru the nearby dielectric between the planes.

    The fact that higher frequencies are successfully
    shunted can be observed in the low magnitude of
    voltage disturbances arising from the impulse-like
    load currents that accompany output edges.
     
  8. Hi guys..

    One more thing..In such a design, is it absolutely necessary to use
    surface mounted caps? Whats the advantage these surface mounted caps
    have over normal ones? We have used only normal ceramics and
    electrolytic caps till now (both on the main board and the RAM board).
    They seemed to work fine on the board, though i cant say anything abt
    the RAM

    Regards

    Mayank
     
  9. That would depend upon what the caps are called upon to do.
    With careful placement of the vias that connect a SMD cap to
    the planes, the inductance can be kept lower than is possible
    when wire leads are attached to a ceramic cap chip. This gets
    the resonant frequency up and the minimum impedance down.
    Of course thru-hole circuits worked for a long time. But the
    advantages of surface mount become ever more important
    as operating frequency and edge speeds go up.
     
  10. Guest

    In general, how was it determine where the cap's needed to be placed?
    What value cap's were choosen?

    I was told to seperate the analog and digital ground. Then tie them
    together
    at the input pins where Vcc entered the board.

    If I tried what you mention it would not work!!!!

    boats_ranger
     
  11. I limit the distance that the bypassed current has to flow
    based on its highest significant frequency content and
    the magnitude of the disturbance I am willing to allow.
    I don't recall. Either 10nF or 100nF.
    Good luck. You'll need it with advice like that.
    It worked for me. In fact, it worked so well that I
    could not observe an degradation of rail noise. It
    changed a little bit in spectrum, but not magnitude.
     
  12. Guest

    I was told to seperate the analog and digital ground. Then tie them
    You have my respect!!!
    Does this imply placing the cap across the shortest distance from it's
    vcc and ground?

    thank's boats_ranger
     
  13. ....

    Yes, provided the referent of your "it" is any one of the
    set of devices generating the currents being bypassed.
     
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

-