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: //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