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

  • From: steve weir <weirsp@xxxxxxxxxx>
  • To: Chris.Cheng@xxxxxxxxxxxx,"'Istvan NOVAK'" <istvan.novak@xxxxxxxxxxxxxxxx>,Chris Cheng <Chris.Cheng@xxxxxxxxxxxx>, si-list@xxxxxxxxxxxxx
  • Date: Tue, 10 Feb 2004 18:54:27 -0800

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:
>//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:
>                 //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:
//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:     
                //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: