Connect with us

How to reduce radiated emissions

Discussion in 'Electronic Design' started by [email protected], Mar 29, 2007.

Scroll to continue with content
  1. Guest

    Hi everyone,
    we have developed a telematics prototype pcb which has to meet the
    class B requirements of EU.It has many cables(like
    RS232,USB,DB15,Audio jacks) connected to it.
    But certain frequencies emitted by the pcb are very high.
    I have tried options like shielding,enclosing with metallic
    box,ferrite cores on the cables etc.. but in vain.
    Can anyone please suggest the effective ways of reducing these
    radiations????
     
  2. Eeyore

    Eeyore Guest

    PCB redesign.

    Graham
     
  3. On 29 Mar 2007 02:27:34 -0700, in sci.electronics.design
    as Eeyore said, pcb redesign, but check out Page 54 in AN70 from
    linear.com, for how to determine what part of the PCB needs attention


    martin
     
  4. There's no panacea-- EMi can spin off in many ways, and some EMi
    reduction methods actually increase EMI squirting out in other ways or
    frequencies.

    One way is to get a braod-band spectrum analyzer, put a tiny one-cm
    loop on the end of the coax cable, and probe around for places that
    generate a peak. Then tackle each peak one at a time, adding ferrite
    beads, bypass caps, or simple series resistors AS CLOSE AS POSSIBLE to
    the active elements. I mean like millimeters. You have to take EMI
    problems slowly, scientifically, deliberately, quantitatively, and one
    peak at a time.

    As other have noted, to really do it right, one often has to redesign
    the lead lengths, bypass cap locations, and ground planes.

    Don't fret too much, many places eventually have to call in an EMI
    consultant, or send the box off to a special EMI measurement and
    abatement place. We have one here in Mn, conveniently placed in a EMI-
    quiet cave, in a quiet valley.
     
  5. Guest

    Been there, done that. Ancient Hacker is right.

    One thing that helped me a lot when I was younger was switching from
    double-sided (two layer) printed circuit boards to four layer boards
    where the two inner layers were devoted to a ground plane and a single
    power plane. Where the two layer board had been barely good enough
    when fitted with a grounded screen plate, the four layer boards
    performed better, even without the screening plate. The are lots of
    other tricks that can reduce emissions and the sensitivity to incoming
    electromagnetic radiation, mostly involved reducing the dimensions of
    the transmitting and receiving loops, and finding them involves the
    slow systematic search that Ancient Hacker talks about.

    Of course, once you have found a few transmitting and receiving loops,
    you do start to get a better feels for low-EMC circuit layout and
    construction.
     
  6. Another good learning method-- tear into a dead TV set-- in order to
    pick up off the air signals they need to have exceptionally good
    shielding of all the radiative areas, which includes almost everything
    except the audio amp.

    Note how they place metal shield boxes over the top and bottom of
    critical areas, how there are ferrite beads on various transistor
    leads, how there's at least a ground copper pour around the single-
    sided PC boards, if not another signal and poured ground layer on the
    flip side..

    In one particularly noisy board I designed long ago, particularly edgy
    signals had to be rounded off by RC filters right at the source
    pins.
     
  7. You need to add split power and ground planes.

    ;)
     
  8. Paul Mathews

    Paul Mathews Guest

    I agree that you are unlikely to pass emissions by merely adding some
    filter components. Books have been written on this subject, and you'll
    find recommendations in previous threads on the same subject. However,
    I'll add a couple of points here:
    1) USB and other differential signaling schemes require absolutely
    balanced lines, over a wide range of frequencies. Any amount of timing
    skew or impedance imbalance results in differential mode EMI, which
    beads and cable clamps will not filter, and the cables are excellent
    antennas at certain frequencies.
    2) Cable quality does matter.
    3) You need to participate in any EMI testing to ensure that the pass/
    fail criteria and apparatus setup are favorable to your equipment and
    to direct the test tech so that data available from the test provide
    you with the most useful diagnostic information.
    4) During testing, you may be required to hook up auxiliary equipment,
    such as a notebook computer. This equipment may have barely passed its
    own radiated EMI tests, and you will be burdened with the field from
    it as well. It pays to find out which auxiliary equipt is most quiet.

    Some search terms for you: Mark Montrose, Keith Armstrong, Howard
    Johnson, minimize loop area, EMI and slew rate control

    Paul Mathews
     
  9. John  Larkin

    John Larkin Guest

    Can you post a picture of the board? What clocks do you have on board?
    And what emitted frequencies are you seeing? There are many
    possibilities here.

    What does the gadget do?

    John
     
  10. Tinfoil hat?

    Good Luck!
    Rich
     
  11. Guest

    Thanks to everyone for your valuable suggestions.
    Please note that ours is a ten layer board out of which 2 are ground,2
    are VCC planes completely.
    we have even taken care of placing ferrite beads,decaps close to the
    chips.What we have observed in our testing is that when we change the
    position of power cable(cable through which power is fed to the pcb
    from a battery) from vertical to horizontal position radiations are
    minimised to great extent.Can anyone please explain why is this
    happening????
     
  12. Fred Bartoli

    Fred Bartoli Guest

    a écrit :
    That's because your board generates some mag field which couples with
    your wire, inducing some voltage along it. Then the wire being a nice
    antenna does its job.

    This is a current loop related problem and to investigate this you need
    an H field probe (small loop on a 50R coax cable end) and an SA.

    But EMI testing on a board along is almost meaningless. For ex. in your
    final product if your box is a metal box (i.e. no coupling to the
    outside world), you might be able to set your power cable path so as to
    minimize the coupling and be done with it.
     
  13. Guest

    You haven't decoupled the power supply carefully enough on the board.

    Every time a logic gate changes state current is drawn from the power
    supply, and flows through the on-board capacitances back into the
    ground and from the back to the power supply.

    If you decoupled the connections to the power supply with a big, low-
    ESR capacitor where they hit the board, most of the high frequency
    current circulates on the board up against your buried ground plane
    and doesn't radiate much. The residual current circulates through the
    pair of cables - power and ground return - that goes to your power
    supply.

    You can minimise this radiation by making your power connection
    completely coaxial - heavy duty coaxial cable and appropriate coaxial
    connectors - but nobody ever does. Twisting the two cables together
    can reduce this radiation a lot, but the terminals on the board and on
    the power supply are always far enough apart to leave two radiating
    loops of significant area.

    You can also reduce the high frequency current circulating through the
    power feed by putting a more elaborate low pass filter structure at
    the power input to the board - but the inductors have to be sized to
    carry the DC current, which means they tend to be bulky and expensive.

    Hope this helps.
     
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

-