Re: [SI-LIST] : PCB design techniques for EMC control

Ron Matthews (ronm@cadence.com)
Thu, 02 Sep 1999 14:19:10 -0700

Hi Steve,

You're right, there's isn't much written about controlling EMI
at
the PCB level that helps people like us fix our problems. Having been
in the EMI mitigation business for about 15 years I can "feel your
pain".

Regarding your list of things to try:

>1. Put a metal can over the offending circuit area.

This can work if you certain your reference plane is quiet. If you put
a can
around a noisey circuit block and refer it to the "ground" plane then it
can
serve to lift the noise on the plane off the board and cause you more
problems than you solved. Do you know what it is in the offencing
circuit
area that is radiating? Will this board ever be offered for sale
without an
enclosure? Are the radiated emissions from the offending circuit
adversely
effecting other circuits on the board?

>2. A separate isolated power plane coupled with a ferrite bead.

Plane segmentation is certainly a valid tool for mitigating EMI in a
PCB.
However, it must be done carefully. Simply using board segmentation
without
considering all the effects it brings with it can be as much of a
damnation
as it can be a salvation if it's done right (Somebody in the choir say
Amen!).

If you're going to create a power plane segment then that segmented
region
should become a routing keep-out for non-related traces that would
otherwise
pass through. If your board is very dense then this may prove
difficult. If
non-related traces are allowed to run freely through an area which has
been
segregated for greater isolation, then these traces will compromise the
isolation you intended the segment to provide.

Using a ferrite to deliver a "filtered" voltage to the segmented area is
a
good idea, but may not give you enough relief by itself. First of all,
make
sure that the ferrite you select has an attenuation characteristic that
will
do what you need it to at the frequencies you need it done at. Once you
have
ensured this, consider putting some shunt capacitance on either side of
the
mote. Select you capacitors to give you the filtering characteristics
needed
given the impedance of the ferrite.

>3. Bead isolated supply for the crystal oscillator only.

Is the oscillator pumping a lot of noise into your power and ground? If
it
is and if the oscillator is adequately decoupled then a bead could
help. My
first inclination would be to take a hard look at the power supply
decoupling
across the entire board, device-by-device.

>4. Separate isolated power and ground plane both isolated with beads.

I'm not sure exactly what you mean here. If you mean to segment the
power
and ground planes for critical circuits then consider the following:

Segmenting both power and ground planes is one of the most aggressive
methods
for dealing with EMI in the PCB. As such, it also needs a great deal of
care
so as not to make things worse. All of the considerations mentioned in
2
above still apply. That is, you have created a routing keep-out in the
segmented region. You also need to aggressively filter the voltage to
your
Vcc segment. However, I absolutely DO NOT recommend connecting your
ground
segment to the main ground plane via a ferrite bead. Remember, a
ferrite
bead has a hig impedance at high frequencies. You want your ground to
be a
low impedance return path. I know of people who will disagree with me
but I
have yet to see any convincing evidence to indicate that connecting
grounds
together through a ferrite is a good thing to do for EMI considerations.

In my opinion, a much better way to go about being successful in
connecting a
ground-plane segment to the rest of the grond plane is to use a span of
etch
which I call a "neck". This is simply a connecting span of etch between
the
segmented ground and the rest of the ground plane. If you consider that
the
ground plane is analagous to a sewer, then this scheme makes sense. The
ground plane in a PCB is like a sewer in the sense that it serves as the
return path for all of the signals created on the board. By using a
neck to
connect a ground sengment to the main ground then you provide this path
for
signal traces which need to enter and leave the segment; which brings me
to
the next thing you should consider if your going to create this type of
segmentation scheme. When you route inter-segment traces, they need to
be
routed over the neck so that the neck can provide a low-impedance path
for
their image return current.

Decoupling is very important in mitigating EMI on the PCB but it is
doubly
important on an isolated segment. If you have an unsegmented
power/ground
plane and if you have done a reasonable job of decoupling the active
devices,
then each device has access to a an "ocean" of charge storage which can
service the switching events occurring around the board. But when you
segment a circuit block on its own separate power/ground island, you are
cut
off from this ocean. As such, you need to be quite aggressive in
decoupling
the active devices on each segmented region.

>5. Separate direct-coupled power and ground plane on the outside layers with
>the signals sandwiched between them.

This is a technique called buried capacitance technology which is
effective
in mitigating some PCB related EMI problems. It's a good technique but
it's
not a panacea. You can get more information on BCT from board
manufacturers
such as Zycon or Hadco.

Good luck,

Ron Matthews Cadence Design Systems

At 04:11 PM 2/18/98 -0600, Lund, Steve wrote:
>Does anyone out there have any good first hand experience of PCB design
>techniques for controlling radiated emissions? I have looked at a lot of
>the available literature and find it does not directly relate to PCB
>design. At this point I am mainly interested in the effects of isolated
>power and ground plane islands around the offending circuitry.
>
>Here is my situation. We have an embedded system in a sheet metal
>enclosure. The PCB occupies an area of about 1 square foot in the bottom
>of the box. The PCB is currently constructed using a continuous power
>and ground plane for the whole board. This board is also utilizing
>through-hole technology (DIP ICs, etc.)
>
>A small part of the circuitry consists of a 110 MHz can oscillator
>feeding a divider chain of 74AC161s. This circuitry occupies an area of
>only 3"x4". Needless to say the harmonics of the 110 MHz oscillator are
>causing our radiated emissions problem. I have looked at the signal
>fidelity in this circuit and it is surprisingly good no doubt to the
>relatively short traces and ground plane.
>
>I would like to try to eliminate as much of this emissions problem at
>the source if at all possible by manipulating the board layout in this
>area. Here are some possible changes that might help the emissions
>problem. Please let me know if you have any experience with these
>techniques:
>
>1. Put a metal can over the offending circuit area.
>
>2. A separate isolated power plane coupled with a ferrite bead.
>
>3. Bead isolated supply for the crystal oscillator only.
>
>4. Separate isolated power and ground plane both isolated with beads.
>
>5. Separate direct-coupled power and ground plane on the outside layers
>with
>the signals sandwiched between them.
>
>Thanks in advance.
>
>Steve Lund
>Emco Electronics
>Slund@tuthill.com
>
>
>
>

**** To unsubscribe from si-list: send e-mail to majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****