Abd ul-Rahman Lomax wrote:

> At 10:09 AM 7/11/01 -0500, Mark E Witherite wrote:
> >At  the 1999 PCB east conference I learned about the 20H rule.  This rule
> >simply put states that EMI can be substantially reduced by keeping the
> >power planes back from the edge of the ground planes by 20 time the
> >dielectric thickness between the two planes.   This would be a lot easier
> >to implement than vias .
>
> This rule of thumb appears to be highly controversial among experts. To my
> knowledge it has never been tested in a controlled experiment. One of its
> effects might be the change in the direction of peak radiation, so a study
> would need to be fairly sophisticated and not just make a measurement in a
> single direction.
>
> Vias are easy to implement. If they are spaced closely enough, which
> depends on frequency, they will essentially complete a ground shield, but
> this may have little effect on radiation except at certain angles. In
> general, where there are multiple ground planes, an increased number of
> vias will be helpful, but one would want these vias not only at edges but
> also close to all potential noise sources.
>
> I simply don't have sufficient experience to know or even make a solid
> guess, and I have never seen a study or even a sufficiently sophisticated
> analysis with a field solver. Perhaps someone else has and my understanding
> is out of date.
>
> Attempts have been made to track back the source of the 20H rule, and it
> does not seem to be much more than a bright idea of one writer; that, of
> course, does not make it wrong.

I'm highly skeptical about this.  I suspect something got lost in translation,
from a specific case, to some general case that doesn't have the special
condition that made it work.  If you figure out the actual AC voltage on a
pair of planes (gnd and voltage supply) in a properly designed, but plenty
noisy, digital board, I suspect it is a couple of mV, maximum.  Now, the way
stuff is generally designed, with 4 layers, or even 6, the power/ground planes
are in the middle, and the signal layers run on the outside.  These signal
traces, although small in area, have 5 V P-P waveforms on them with
VERY fast edges, therefore a frequency spectrum that runs much higher
than the mushy signals on the power planes.  The decoupling caps as well
as the large area intrinsic capacitance of the planes are going to keep
the spectrum of the plane voltages down to the lower frequencies.
Also, the loop areas of some of the signals where significant current pulses
ocurr at the transitions will be much more efficient radiators than the
several mil gap between the planes.

Now, there are a whole bunch of issues with cuts in power planes that
create slot antennas, but that is a different phenomena.

But, I think the whole thing came from a mil-spec board with grounded planes
on the outside, and LOTS of layers of high-speed signals running around
BETWEEN the planes.  This turns the area inside the planes into a complicated
waveguide.  Although such a waveguide would be pretty lossy, it is conceivable
that substantial signals could make it to the edge of the board and be
radiated.
Changing the edge so that one plane ends and the other continues may cause
the signals to be 'dumped' into the continuing plane.  Closing the edge up with

a bunch of vias might even be better, but if you had one plane grounded, and
one a power plane, you can't just stitch them together, you'd need capacitors
there.  Anyway, the waveguide beyond cutoff effect would seem to make such
a scenario only function in the  millimeter wave band, and even microwave
PCB dielectrics are massively lossy up there, so I'm still skeptical about
whether
this was a practical discovery, or something that was predicted from a
simulation
run by someone who really didin't understand the practical performance of
the materials used.  I rather suspect the latter to be the case.

One possible explanation, which includes a number of special conditions, goes
like this:  The board is in a card rack, with metallic card guides.  The card
rack is poorly designed, so the card guides couple electrically to the cabinet
exterior.  The power planes carry digital noise to the card guides, and thus
to the cabinet exterior, where they are seen in an EMI test.  Now, of course,
once the solder mask is worn off by the card guides, the whole power supply
shorts out!  Using metallic card guides which wipe over powered conductors
on the board is a design error far greater than a little EMI!  But, this is the

kind of scenario that could have passed through word-of-mouth a dozen times,
and become a designer's mantra somewhere.

Jon

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*                      - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to