[SI-LIST] Re: Stack up for EMI reduction, plane resonance and u-s trip radiation etc etc

Chris, Steve, Nima,

Jumping into the middle of the discussion...  some thoughts on a number of 
comments/
subjects brought up... including the original one...

First, Nima....
The information you've given is not really sufficient to give any of us 
sufficient grounds
to base many of the presuppositions that have been offered.  A lot of the 
ideas offered
are certainly possible but giving us a stackup and a few frequencies is not 
enough
to draw a certain conclusion.  I think someone early on said something to 
that effect.
I've arrived at a test site to look at a client's product issue and it 
usually starts with the
information that you've supplied.  There's a lot more to know in order to 
put a problem like
that to rest.

I have several questions that I hope will help you:

1.  Are we talking a single board or multiple boards?  Anything else 
notable about the system
that might contribute to the problem?
2.  Have you proven that it is related to the 700 MHz signals?  Are there 
any other
operations on the board that might generate these?
3.  How does the radiation problem manifest itself?
4.  What has been done that hasn't worked?
5.  Are we talking about broadband noise or all harmonically related signals?
A comment you made suggested that there might be other signals present also.

Just a suggestion:  Don't just change a stackup just because there is 
nothing else you
know to do.  You'll need to do a lot more detective work to solve this and 
if you still
can't get it, let us know what you found out and maybe we can help you more.

Various comments/subjects found in the thread...

re: "Any HF noise that resonates in the planes can find its way out, by 
going up
vias to some structure above the board."
Yes.  When this propagates outside the system, this is known as "common mode"
radiation... a very nasty and difficult problem to solve on the whole.  It 
is such because
everything tied to that common point, a plane usually "ground", will be 
energized as
"one" making it difficult to track down the real culprit causing the 
problem.  Common
mode radiation is not the same as "plane resonance", though.  A resonance 
implies
that a "standing wave" is present in some form.

re: excessive power/ground/signal pins... (understood to be plane 
perforations, etc.)
That's almost always causes a real nasty problem that will cause common mode
radiation.  Hence, my next point...

re: EMI reduction (in relation to components on PCB and the PCB itself)
It is the package that radiates and it does so against the reference which
is the PCB to which its attached.  If the local reference inside the chip is
at the same (or very nearly the same) potential as the PCB underneath it, 
there
will be little or no radiation to speak of unless there are other issues 
left unresolved.
No stackup can fix this by itself unless the potential between the elements 
of the
problem is brought to very low levels or effectively "zero".  The key here 
is to reduce the
PCB to package impedance at the spectrum of interest.  But this is not 
"news", this is
EMC 101. Examine the ways to reduce that impedance and you'll have the 
solution to
fixing the problem...and you'll be on your way to fixing the decoupling 
issue we all talked
about a few weeks ago as well.

re: plane resonance
Fortunately, all the things necessary to make these problematic are not 
present in
most instances.  In fact, it is my opinion (because I haven't proven it but 
it would seem
to be true), that they cannot be entirely eliminated.  They can only be 
mitigated.  The best
we can usually do is make sure that the driving impedance into the resonant 
circuit is
much lower than the driver can "drive" at the circuit's resonant 
frequency(ies).  This means
that close power/ground plane spacing is appropriate to help prevent these 
as it drives up the
capacitance which drops the "differential mode" power structure 
impedance.  It is also a
reason why extensive PCB grounding with close PCB spacing to the chassis 
does the same
in the "common mode" sense.

re: ustrip radiation
All things equal, a microstripline will radiate more effectively that a 
stripline. A study of
the field lines surrounding these structures should show why.  That is not 
to say that
the microstrip will always be a problem, though.   Well designed 
microstriplines should
perform well but at times may require more "peripheral field containment" 
than a well-designed
stripline.  It is a matter of the skill used in the design of each and what 
sort of signals are
presented upon them that determine whether they will be a problem or 
not.  In summary,
microstriplines are not inherently bad to use but they might at times take 
a bit more care
in using them under certain circumstances.

re: "Ans : Beaten to death, package is the choke point. EMI noise radiates 
from package not PCB"

Almost but not quite true.  The package does seem to be a problem but to 
eliminate the PCB from
culpability is not totally accurate.  Structures very similar to the 
package problem can exist in
PCB designs and the effect is the exactly same but usually at lower 
frequencies.  Folks on the whole
are getting better at this avoiding this and it doesn't show up as much 
these days but it can and does
happen.  Just think of the PCB just being a "macro" version of the package.

re: " Ans : Managing the return path and reference plane not the decoupling 
caps"

Again, almost but not quite true.  While managing the return path and 
reference planes are vital in
these matters, so is managing your power that supports these signals.  What 
is not generally
realized is that when a chip is "starved", its waveform changes and the 
driver may experience
instability and generate signals at much higher frequencies than 
expected.  That sad truth is that
you have to manage the signal, the signal path and return, and all energies 
used to produce and
propagate the signal.

Best Regards to all,

Michael E. Vrbanac



At 08:08 PM 2/10/2004 -0800, you wrote:
>Steve,
>I believe excessive power/ground/signal pins to support for I/O on Larry's
>package is the cause of the perforation. I could be wrong though.
>Chris
>
>-----Original Message-----
>From: steve weir [mailto:weirsp@xxxxxxxxxx]
>Sent: Tuesday, February 10, 2004 6:54 PM
>To: Chris.Cheng@xxxxxxxxxxxx; 'Istvan NOVAK'; Chris Cheng;
>si-list@xxxxxxxxxxxxx
>Subject: Re: [SI-LIST] Re: Stack up for EMI reduction, plane resonance
>and u-s trip radiation etc etc
>
>
>Chris,
>
>Any HF noise that resonates in the planes can find its way out, by going up
>vias to some structure above the board.  USF had some interesting data on
>this that I saw a few years back.  Also, depending on whether a fence has
>been used, noise can couple out at the board edges.  The best that I know
>of is that we can detune the board from the excitation by a combination of
>via and caps for that purpose, provided the board impedance is not too low
>to be able to do anything.
>
>Maybe I misunderstood, but I was under the impression that with Larry's
>package they had added pins to try and hold the cut-off frequency up, so as
>to limit the amount of in package capacitance needed in those really high
>current devices.  The side effect was that this chewed up the planes
>necessitating making the impedance on that side of the interface nasty.  So
>they got stuck with the thin, high K dielectrics that made the boards
>resonate at a low frequency.  I believe that the comment Larry offered was
>a general one that he had not seen package cut-off below 20MHz or much
>higher than 100MHz.
>
>Regards,
>
>
>Steve.
>At 06:18 PM 2/10/2004 -0800, Chris Cheng wrote:
> >OK,
> >My feedback :
> >a) Yes package resonance varies, in fact if I understand Larry's previous
> >comments, his package has so much perforation on the PCB that it has choke
> >points BELOW 100MHz. He has to use thin core just to bring the resonance
> >back to near 100MHz. My question is what will be harmed by the noise leaked
> >out to the system beyond the choke point ? It is a chicken and egg problem,
> >if nothing from the PCB side can bring in help to sustain the core noise
> >margin, nothing from outside can bring enough harm to impact the core
> >neither. What remains "harmful" is an EMI containment problem (through
>plane
> >stitching) and not a decoupling issue.
> >b) The plane capacitance is used for the image current of the non-ground
> >reference plane to AC coupled to the ground on the other side that the
> >stripline signal is referencing. It is a function of the etch rate and
> >locality of the signal.
> >c) If you can measure a converter that can provide "harmful" level of noise
> >to the silicn core supply, I think the last thing you worry about is
> >decoupling solution. You should fire the converter vendor. If it is what
>you
> >call "meet all the other functional spec", it falls back to EMI containment
> >rather than decoupling.
> >
> >At the end of the day, throwing fancy caps or thin core is still neither
> >necessary nor the most effective.
> >
> >
> >-----Original Message-----
> >From: Istvan NOVAK [mailto:istvan.novak@xxxxxxxxxxxxxxxx]
> >Sent: Tuesday, February 10, 2004 5:55 PM
> >To: Chris Cheng; si-list@xxxxxxxxxxxxx
> >Subject: Re: [SI-LIST] Stack up for EMI reduction, plane resonance and
> >u-strip radiation etc etc
> >
> >
> >Chris,
> >
> >See my comments below.
> >
> >Regards,
> >
> >Istvan Novak
> >SUN Microsystems
> >
> > > Istvan,
> > >
> > > You got me on this one, I really need to figure out where can the
> >200-400MHz
> > > noise on PCB comes from ?
> > > Is it :
> > > a) Core noise, IC internal switch noise which propagate through the
> >package
> > > power pins to the PCB
> > > Ans : Beaten to death, package is the choke point. EMI noise radiates
>from
> > > package not PCB
> >
> >Are you sure that the resonance frequencies of the package and PCB are
> >always exactly
> >the same?  If the PCB resonance lines up with the excitation frequency,
> >while the
> >package structural resonances dont, a relatively large attenuation through
> >the
> >package-board interface still cant block harmful radiation from the board
> >(before you ask: such situations were measured on real boards).
> >
> > > b) I/O switching noise, comes out from signal pins needs a return path
>the
> > > I/O power
> > > Ans : Managing the return path and reference plane not the decoupling
> >caps.
> > > Yes, the plane CAPACITANCE not inductance provides the return path for
>the
> > > image current return through the opposite reference ground plane.
> >
> >Capacitance or inductance and thin laminate: OK lets ask a different
> >question.
> >You say you need plane capacitance.  Is the required amount of plane
> >capacitance
> >independent of how many traces the plane has to reference?  Do you want
> >more plane capacitance if the same plane area references faster and more
> >traces?
> >
> > > c) External terminators,
> > > Ans : The resistance of the terminator is the damping factor
> > > d) Noise from the supply
> > > Ans : 200-400MHz noise from a supply ??????
> >
> >Several hundred MHz noise may come from the converters, though
> >I agree that if a converter does that it is not the best converter, but it
> >still
> >can meet all the other functional spec (and again: it was measured on
> >real parts).
> >
> >
> > > e) External cable coupling
> > > Ans : ferrite beads and chokes
> > >
> > > Aside from the above, none of which is related to fancy decoupling caps
>or
> > > thin core PCB, where else ?
> > >
> > > Chris
> > >
> >
> >------------------------------------------------------------------
> >To unsubscribe from si-list:
> >si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
> >
> >or to administer your membership from a web page, go to:
> >http://www.freelists.org/webpage/si-list
> >
> >For help:
> >si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
> >
> >List technical documents are available at:
> >                 http://www.si-list.org
> >
> >List archives are viewable at:
> >                 http://www.freelists.org/archives/si-list
> >or at our remote archives:
> >                 http://groups.yahoo.com/group/si-list/messages
> >Old (prior to June 6, 2001) list archives are viewable at:
> >                 http://www.qsl.net/wb6tpu
> >
>
>------------------------------------------------------------------
>To unsubscribe from si-list:
>si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
>
>or to administer your membership from a web page, go to:
>http://www.freelists.org/webpage/si-list
>
>For help:
>si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
>
>List technical documents are available at:
>                 http://www.si-list.org
>
>List archives are viewable at:
>                 http://www.freelists.org/archives/si-list
>or at our remote archives:
>                 http://groups.yahoo.com/group/si-list/messages
>Old (prior to June 6, 2001) list archives are viewable at:
>                 http://www.qsl.net/wb6tpu
>


------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List technical documents are available at:
                http://www.si-list.org

List archives are viewable at:     
                http://www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu

Other related posts: