MC, how are you going to reduce inductance other than by reducing plane separation? Regards, Steve. At 10:22 PM 2/11/2004 -0600, lenaw wrote: >Istvan: > On (b) my opinion is that if you want to reduce the power/ground >bounce, you have to reduce the total effective inductance of the >power/ground planes ( assume you have no bond wire and use flip-chip >technology to connect the die to the package ) and it depends on what kind >of buffer technology you are using, signals on top of a pair of closely >coupled power/ground reference may not be the best solution because you need >the strong mutual inductance between the signal and power or ground planes >to reduce your total effective inductance during SSO. Just my 2cents. > > >Regards, >MC > >----- Original Message ----- >From: "Istvan NOVAK" <istvan.novak@xxxxxxxxxxxxxxxx> >To: "Chris Cheng" <Chris.Cheng@xxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx> >Sent: Wednesday, February 11, 2004 9:59 PM >Subject: [SI-LIST] Re: 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 > > > >------------------------------------------------------------------ >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