Chris, OK, time to stop the thread. Regards, Istvan ----- Original Message ----- From: "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx> To: "'Istvan NOVAK'" <istvan.novak@xxxxxxxxxxxxxxxx>; "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx> Sent: Thursday, February 12, 2004 4:13 PM Subject: RE: [SI-LIST] Stack up for EMI reduction, plane resonance and u-strip radiation etc etc > No,no,no. We are not in agreement. Especially you haven't answer my question > : > "how could your fancy capacitor or thin core plane help if they are > electrically further from the reference planes ? " > > First of all, you can't get into the power and ground bounce issue with the > reference planes without getting into crosstalk problem. Afterall, it is > the constructive overlapping of the image current that creates the > power/ground bounce problem in the first place. > > Now let's think about what do you need to do to bring in the thin core > decoupling plane to relief the problem. You first need to drill vias to > bring the image current from the reference power plane to the other side of > the power plane that has the thin core capacitor. The current then has to AC > coupled to the ground plane through the thin core and then come down to the > ground reference plane with additional ground vias. This is not a low > impedance path as compared with direct plane coupling and the vias has to be > numerous and very close to the signal traces to be effective. Here comes the > problem, if your signal traces are so close that the image current starts to > overlap on the reference already, WHERE ON EARTH DO YOU FIND THE SPACE TO > DRILL THE NECESSARY VIAS ? > Like I said before these power/gnd bounce problem on signal trace crowding > is an observable problem on highspeed high density package. I have done > enough of these packaging analysis to convince myself your trade-off point > does not exist. i.e. Either your traces will be so spaced out that vias can > be drilled near but then their image current don't overlap each other > significantly on the reference plane to create power/gnd bounce problem OR > they will be so tight and close that you can't drill your via to bring in > your thin core relief current anyways. > > And for the last time to answer your last question. The spacing between the > signal/power/gnd planes are dictated by the impedance control parameters. It > is not dependent on the edge rate of the signals. > > What I am disappointed and alarmed is all these discussions/arguments has > been repeated over and over in this forum and if you go back to the archive > a few years back, there was a flare up with exactly the same argument and I > have pointed out exactly the same problem. Did anything changed since then ? > I certain have not changed your mind and neither have I so what's the point > of continuing this discussion ? > > > -----Original Message----- > From: Istvan NOVAK [mailto:istvan.novak@xxxxxxxxxxxxxxxx] > Sent: Wednesday, February 11, 2004 7:59 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, > > > a) If your plane reference is so limited and crowed with highspeed traces > > that it can not provide the effective capacitance, it will exhibit itself > as > > both xtalk and power/gnd bounce problem. The image current starts to > overlap > > each other and either add or subtract from each other. This is an > observable > > problem in most signal traces in organic packages. But I will turn the > table > > around and ask you, how could your fancy capacitor or thin core plane help > > if they are electrically further from the reference planes ? It's like > > challenging my Covertte saying "hey, I bet you can't drive this car at > > 300mph" while you are sitting on a pintle. > > So I think we are in agreement here that if trace density is increases, > beyond > a certain point we will have power/ground bounce issues on the planes. > You are correct that crosstalk among traces will probably go up at > a similar rate, but it is a matter of system design, which will pose a > limitation first. > If you hit the power/ground bounce limit first, and crosstalk is still not > harmful, > a thinner power/ground laminate may help to reduce power/ground bounce. > If in the new stackup you still reference the same power plane, what has > changed is that the traces will be 'outside' of the power/ground cavity, not > inside as before. In this case only the ground reference plane for the > traces is > what is further away from the power/ground plane pair. If the components > on the board force you to have a large number of ground vias anyway, you > can get the sufficiently tight stitching between the ground planes without > extra > expence. > > > > b) At extreme high edge rate, the skin effect is limiting both the signal > > trace and the image current that flows on the reference plane, your > infinity > > argument doesn't exist. I can't answer an argument that cannot exist. > > OK, let me rephrase the question that may be easier to answer. Say you > have a working board, and you are satisfied with it. It has a given number > of traces referencing the correct plane. Say the transition times on those > traces are all around 1 nsec. And lets suppose the power/gnd bounce > is acceptable: not much lower than your target, but safely below your > limit. Suppose the only thing you change next is the silicon, and it puts > out > 200psec transition times instead of 1nsec. There is no other change > on the board. > The 200psec edges are 'slow' enough that within an inch radius we cant > really > expect any absorption due to skin effect, and the one inch radius > approximately > represents the distance the signals can go within 200psec. So the > question is: if you want to maintain about the same level of power/ground > bounce, > would you change the plane structure; would you put the power/ground planes > closer, further apart, or leave them where they are? > > Regards, > Istvan > ------------------------------------------------------------------ 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