Connect with us

ground plane connections

Discussion in 'Electronic Design' started by Jamie Morken, Nov 20, 2004.

Scroll to continue with content
  1. Jamie Morken

    Jamie Morken Guest

    Hi all,

    When using a high frequency (1MHz to 3MHz) stepdown buck switcher on a
    board to generate the 5Volt rail, what is the best way to connect the
    switchers ground plane to the rest of the 5Volt ground plane? Is a
    single point connection good to use to reduce noise, or is it better
    just to make one big ground plane under the switcher circuitry and the
    5V circuitry?

    Jamie Morken
  2. Leon Heller

    Leon Heller Guest

    The switcher chip manufacturers usually have recommended PCB layouts.

  3. John Larkin

    John Larkin Guest

    Just one common plane for the whole board is usually fine, unless
    you're doing very low-level stuff. Keep the low side of the input cap,
    the anode of the catch diode, and the low side of the output cap very
    close to minimize broadcasting the circulating switching current about
    the plane.

    Some people like to cut a c-shaped relief in the ground plane and tuck
    all the switcher parts on the resulting peninsula to keep circulating
    currents out of the rest of the plane, but that's not normally needed.

    What else is on the board?

  4. Ken Smith

    Ken Smith Guest

    It depends a great deal on what the rest of the board has on it and what
    it hooks to. In digital logic cases it is almost always ok to just hook
    the switcher stuff straight to the boards ground plane.

    If the circuit has analkog stuff or something else that can be disturbed,
    you want to make sure that the AC currents all stay local to the switcher
    section. This is usually done by careful parts placement adn perhaps
    using a layer of the PCB as an extra ground layer.

    ------+----/ 0---+----))))))------- To load
    ! !
    --- ---
    --- ^
    ! !
    +---------- Local plane or careful placement
    --------+-------------------- PCB ground plane

    In extreme cases where you have very small signals near the switcher, it
    is best to layout as though you will be adding a shield. It costs almost
    nothing extra in the board design and if it turns out you need the shield,
    you have a place to put it. I have resorted to having the switcher on its
    own plane above the PCB's ground plane and running all the lines in and
    out through inductances. It sort of like this:

    ........ Shield ............
    . .
    . ------------ .
    Vin -+-[L1]-+---! Switcher !----+--[L2]-+---- Vount
    ! . ! ! Circuit ! ! . !
    --- . --- ------------ --- . ---
    --- . --- ! --- . ---
    C1 ! . ! C2 ! C3 ! . ! C4
    ! . ---+-----+--------- . !
    ! . ---+ . !
    ! ....!.[L3].................. !
    ! ! !
    ---+----------+-----------------------+--- GND

    L1, L2 and L3 are all on the order of 1uH and are lossy.

    The impedance of L1 forces the AC current to flow in C2. You can't use a
    large inductance here because larger inductors have too much stray
    capacitance. You must maintain a high impedance at high frequencies. L1
    also reduces the conducted EMI on the input power.

    L2 serves very much the same purpose as L1. From an EMI point of view it
    usually matters less than L1. From a circuit performance, it often
    matters more.

    L3 is a bit of an oddity. If the shield is used, the drops caused
    by ground currents will tend to drive it with an AC waveform. The
    losses of L3 prevents the shield from tuning up at some frequency.
  5. Joerg

    Joerg Guest

    Hi Jamie,

    One big old common ground plane is what I found to work best for most of
    my designs. And also for those that I had to redesign. This included one
    design where the switcher provided 5V at up to a whopping 100 amps.

    However, it helps to still adhere to Ken's advice of keeping currents as
    local as you can. That means not placing the inductor too far away from
    the FET. The same goes for the path to decoupling caps, Schottkys and so
    on. In other words anything where high currents are abruptly changing
    their path. With regard to noise issues decoupling caps have to be seen
    as the 'real' power supply in switchers since that is where almost all
    the short term energy gets drawn from or is dumped into.

    Regards, Joerg
  6. Clarence

    Clarence Guest

    The decision for splitting the ground depends largely on the peak currents.
    For most of the low powered switchers a large common ground plane is preferred,
    as long as the switcher is grouped for the shortest spacing so as to localize
    the currents and minimize the IR drops. For really high currents, say over 10
    amperes, you must consider the current path on the board and decide whether to
    group and split the ground plane to limit influence from the high peak

    Remember a single point connection has a finite resistance which must be
    minimized to avoid heating the board.
  7. Joerg

    Joerg Guest

    Hi Clarence,
    Also, don't send lots of amps through one lone via until it gloweth in
    the dark ;-)

    Regards, Joerg
  8. Terry Given

    Terry Given Guest

    Damn, here I was thinking Copper is a room-temperature superconductor. doh.

    You can work out the current-carrying capacity of vias by assuming the
    via wall thickness is 1/2 that of the pcb copper cladding.

  9. Clarence

    Clarence Guest

    Oh yes! Or char the board!
    For surface mounts in even a relatively low powered buck regulator I often use
    six vias for the caps, and at least the same for the diode. The vias for this
    purpose are larger ones, not .01 In Dial, if space is available I want them
    more like .03 dia to get more plating.

    However the "single" point may be one entire side of the circuit area with only
    a narrow isolation on three sides. This arrangement will still avoids the
    currents in the supply being in the ground circuit of other portions of the
  10. Clarence

    Clarence Guest

    So a minimum of two for each pass through would be the minimum to use. I
    prefer four to six! Also the circumference of the via must be more than the
    land connecting it to the circuit. Higher currents require many more....
  11. Terry Given

    Terry Given Guest

    Ayup - cant argue there. bigger holes = greater circumference. Dont tent
    the vias if the pcb is wave-soldered, the solder will help too.

    At the 200A level one uses rather a lot of vias. Aint 10 Oz pcb's great.

  12. Joerg

    Joerg Guest

    Hi Terry,

    Another issue to watch out for are thermal reliefs. That is not so much
    of a problem these days anymore but I remember cases where this data was
    separate from the rest. Then PCB manufacturers occasionally defaulted to
    thermal reliefs in high current vias that were meant to provide a low
    impedance connection but no component mounting.

    Regards, Joerg
  13. Terry Given

    Terry Given Guest

    Hi Joerg,

    I am in the habit of putting a sentence along the lines of:

    "No copper to be added to or removed from the design"

    into the PCB spec sheet, as well as telling the manufacturer not to do
    so. Several manufacturers have in the past helpfully placed things like
    logos, UL ratings etc. on areas deliberately left blank - for HV
    creepage/clearance necessary to comply with safety standards :(

    If the artwork needs fiddling, I'll fiddle with it thanks. Step and
    repeat all you want, drill holes whatever size you like as long as the
    finished diameter is as spec'd, but leave the copper alone.

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