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

Ron Matthews (ronm@cadence.com)
Thu, 19 Feb 1998 11:22:21 -0500

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
>
>
>
>