Content-type: text/plain; charset=US-ASCII
Subject: Re: [SI-LIST] : PCB design techniques for EMC control
Date: Wed, 18 Feb 1998 21:58:07 EST
Organization: AOL (http://www.aol.com)
Content-type: text/plain; charset=US-ASCII
In a message dated 2/18/98 5:59:59 PM EST, SLund@tuthill.com writes:
<< 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.
***I have quite a bit ( about 17 years: seams like for ever.... ). You are
somewhat correct in saying not a great deal of litrature exists on reducing
EMC, at the moment it's still not "public domain" and folks want paying for
it. The SI list is mainly SI folks, with a few having EMC experience too. I
wrote an artical in PCD magazine addressing ground plane penatrations(?) that
may help you too. Now, on to your problem.***
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.)
***I would hope that your circuit is not tied to the box in any way. If you
allow current to flow in the chassis, it may never be possible to reduce the
emission enough to meet the spec. You don't mention how power is supplied to
the circuit. This is one of the major links in the path of the current that
causes the radiated emission.***
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.
***Before you conclude that it's the oscillator that's your problem, those
drivers move an awful lot of current each time they switch. Is there a way
that you could run just the oscillator with it driving a SM resistor rather
than the 74 AC logic? This would help you isolate the source a bit more. Often
with DIPS you can lift a pin and add the resistor.
I think you should co-locate all this circuitry on your board. I am assuming
that you have good decoupling on each device with minimum loop area etc. Is it
possible that this circuitry could be on a sub-board which could be filtered?
A guess that my own experience is that you could Micro-Island the entire
circuit. If you do this, supply POWER to the island using a filter that has
common mode impedance. A simple filter with just the +ve lead filtered will
not eliminate the harmonics from propagating out through the power supply. I
would apply filters ( distributed LC ), not just beads, at the point where you
signals leave the Island. I've seen Fe beads or FT caps make the situation
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
1. Put a metal can over the offending circuit area.
*** Good if the chips and traces were radiating, but I would not start here...
You still have the problem that the noise is carried out on any traces that
leave the area.***
2. A separate isolated power plane coupled with a ferrite bead.
*** I've used this with limited success, but see the comments about common
3. Bead isolated supply for the crystal oscillator only.
***Could work, but typically the crystal is very low power. I would look to
the output stages in the AC logic as the culpret first... ***
4. Separate isolated power and ground plane both isolated with beads.
***Could be a very good approach. You need to make sure tha the impedance in
the ground plane does not screw up the SI. That's why I suggest using a CM
5. Separate direct-coupled power and ground plane on the outside layers
the signals sandwiched between them.
***This is difficult from a practical point of view. I also have reservations
about forcing current to change sides of a plane often. One of these days I'd
like to see an analysis of how current flow in this situation... Do you know
Thanks in advance.
*** Just a plug for my business, I have a small EMC design and test facility
just outside Chicago. If your having problems trying to meet the EMC
requirment, perhaps we could help you figure it out. We have many diagnostic
tools, EMSCAN, Close field probes etc...
I also have an e-mail in Acrobat format, if you would like I could add you to
the mailing list.***
Very best wishes,