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

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
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.
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 ??????
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

-----Original Message-----
From: Istvan NOVAK [mailto:istvan.novak@xxxxxxxxxxxxxxxx]
Sent: Monday, February 09, 2004 7:58 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,

Well, it depends on the nature of the devil; if you are
concerned by noise getting from the PCB into the
package through its power/ground pins, you are
correct: the package resonance will filter out noise
above the cutoff frequency.  If you also want to
reduce the noise on the PCB itself, the active devices
will not reduce the noise for the same reason, because
the package separates the silicon from the PCB.

Regarding parallel plate capacitance: this was discussed
several times on the list, and I dont want to repeat
myself.  But I think we are saying the same thing.
When you say parallel plate capacitance, I say
inductance.  For a board of a few inches in size or
bigger, the lowest series resonance of the board plates
is 100MHz or lower. Above that frequency the impedance
is mostly inductive.  If you need a certain amount of parallel
plate capacitance, we like it or not, it comes with a certain
amount of inductance above the series resonance.  If
you need more parallel plate capacitance, you get it
together with lower inductance.

Regards,

Istvan Novak
SUN Microsystems

----- Original Message -----
From: "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx>
To: "'Istvan NOVAK'" <istvan.novak@xxxxxxxxxxxxxxxx>; "Chris Cheng"
<Chris.Cheng@xxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx>
Sent: Monday, February 09, 2004 4:33 PM
Subject: RE: [SI-LIST] Stack up for EMI reduction, plane resonance and
u-strip radiation etc etc


> Yes, once again the devil is in the details. It is one thing to stick an
> impedance probe to measure the power plane impedance at a random location
on
> the PCB. It is another thing to measure it on the real load side (i.e.
after
> the package). Have you done that ? Are you convince you can even see any
> effect at 200-400MHz on PCB through the package ? Your colleague Larry and
> me don't think so.
> As for I/O return current related noise on PCB, it is the parallel plate
> capacitance that sandwich the stripline which is responsible for the
> decoupling/return of the current (at least at 200-400MHz). Not the thin
core
> power/gnd pairs or fancy decoupling caps.
>
> -----Original Message-----
> From: Istvan NOVAK [mailto:istvan.novak@xxxxxxxxxxxxxxxx]
> Sent: Sunday, February 08, 2004 3:07 PM
> To: Chris.Cheng@xxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
> Subject: Re: [SI-LIST] Stack up for EMI reduction, plane resonance and
> u-strip radiation etc etc
>
>
> Chris,
>
> I am not speaking for Zhangkun, but in many of the real boards I have
looked
> at by measurements and simulation, you can see the evidence of
antiresonance
> between the plane capacitance and inductances of capacitors.  Chips (at
> least on those boards I have looked at) did SHIFT the resonance frequency
> slightly, but did not make the peak go away.  You are correct in saying
that
> if you sprinkle the board with capacitors, the resonance peak is
suppressed.
> But as you said in one of your recent postings, the devil is in the
details:
> sometimes you may need so MANY capacitors over the board area to
> sufficiently suppress the resonance that it becomes a pain.
>
> Regards,
>
> Istvan Novak
> SUN Microsystems
>
> ----- Original Message -----
> From: "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx>
> To: <si-list@xxxxxxxxxxxxx>
> Sent: Monday, February 02, 2004 10:15 PM
> Subject: [SI-LIST] Stack up for EMI reduction, plane resonance and u-strip
> radiation etc etc
>
>
> > Finally......
> >
> > Zhangkun,
> >
> > I am also curious about these 200-400MHz plane resonace. If you sprinkle
a
> > PCB with a wide range of caps with different values and at different
> > location and with high power loading (ie real IC chips) at different
> > location, do you still see pronounced peaks at 200-400MHz ? I have no
> doubt
> > a bare power/gnd plane pair can resonate at those frequencies, but I've
> > never seen that case once realistic caps and loading (IC chips) is
placed
> on
> > the PCB. Are these simulation results or measurements based on a real
> system
> > with chips and caps ?
> >
>
>
------------------------------------------------------------------
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: