Chris, as I said, I view it as an EMI, not power concern. That could change on large boards, particularly with high K materials as lamda / 2 gets down below the IC PDS cut-off. Regards, Steve. At 05:46 PM 2/10/2004 -0800, Chris Cheng wrote: >Steve & Ray, >Good point, there will be noise leaking out from the core through the >package. It will be "grossly inadequate" or attenuated to not affecting back >into other chips core through their package. So is this a matter of >containment or decoupling ? Like you said below, a nice faraday cage formed >by top and bottom ground planes stitched with ground via may just be as >effective as your decoupling solution. >Is it the wild Von Karmann wind that can knock the bridge off or the blow >that takes out the birthday cake candle ? >I believe it's just the later. > >-----Original Message----- >From: steve weir [mailto:weirsp@xxxxxxxxxx] >Sent: Tuesday, February 10, 2004 2:13 PM >To: Chris.Cheng@xxxxxxxxxxxx; 'Istvan NOVAK'; Chris Cheng >Cc: si-list@xxxxxxxxxxxxx >Subject: Re: [SI-LIST] Re: Stack up for EMI reduction, plane resonance >and u-s trip radiation etc etc > > >Chris, > >There is one point that I disagree on. Even though the package cuts off >with at least a -2 slope, there is quite of bit of high frequency energy >that still passes between the PWB and the IC. It is just grossly >inadequate to power the IC. But it has lots of potential to aggravate EMI >problems. > >No one believed Von Karmann when he theorized that wind was the source of >energy that sent the Tacoma Narrows bridge into destructive >resonance. But, we all have learned that Von Karmann was right. > >So now we have these resonant cavities in the form of PWB's with very low >damping coefficients. The IC's don't provide much damping, because as you >note the packages appear reactive, not resistive. As long as the energy >stays in the cavities and sloshes around at frequencies higher than the IC >cut-off(s), it probably isn't any big deal. But we have these: board >edges, vias, and components, all more than willing to provide radiation >paths for that energy. > >One of the hotter debates was the 20H rule. Amidst that debate came the >notion of ground fences on the outside of the board. While I like those >for ESD, they can do just as much harm as good for EMI. > >At 01:22 PM 2/10/2004 -0800, Chris Cheng wrote: > >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 > >Agreed > > >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. > >This is where as system integrators, we end-up applying band-aids due to >poor IC design. > >Minor nit, I disagree with your characterization of plane >capacitance. Sure, without capacitance we would not have a coupling >mechanism, but at the frequencies of interest, the behavior over even >fairly short distances is of a transmission line, not a capacitor. This is >especially true with high K materials, and thin laminates. > > > >c) External terminators, > >Ans : The resistance of the terminator is the damping factor > >Agreed. > > >d) Noise from the supply > >Ans : 200-400MHz noise from a supply ?????? > >It's all those TWT's that they like to use in quarter bricks!!! ( Just >kidding, everyone knows it is the Klystrons. ) > > >e) External cable coupling > >Ans : ferrite beads and chokes > >Moating near I/O, shunt devices such as feed-through caps, or X2Ys are >pretty effective too, adequate bonding of the PWB to the chassis, etc. > > > >Aside from the above, none of which is related to fancy decoupling caps or > >thin core PCB, where else ? > >It is a matter of impedance. Either we get the decoupling capacitors >significantly closer to the package than lambda / 4, or we have stuck the >characteristic impedance of the planes between the IC and the caps. For >thick dielectric where that impedance can be an ohm or more, that is often >way too much. So, get close, or pay for fancy thin dielectrics. > >What fancy decoupling capacitors can do is make it easier to stay close to >the IC by using fewer devices. But we are still stuck drilling enough via >holes to attach those devices. > >Steve > > >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: > >//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 > ------------------------------------------------------------------ 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