Zhiping - Voltage is always with respect to (WRT) some other node. All voltages on printed circuit boards, electronic packages or chips are differential. Voltage is the potential of one node WRT another node. We sometimes talk about the voltage of a node WRT the center of the earth or WRT spice node zero (they are the same thing) but those voltages are irrelevant for signal integrity in our products. The only thing that counts is the difference in voltage between two nodes, for example a signal WRT local ground. For traces in a PCB, the difference voltage is always vertical, the voltage of a trace WRT the local reference plane. TEM mode analysis is good for all the stuff we do. The PCB stackup in question has ground planes that surround both the analog and digital traces. The only thing that is important is the differential voltage between the trace and reference (ground) planes. That difference voltage will propagate down the trace (transmission line). Eventually, the voltage/current waveform will arrive at a via that takes it to the surface of the PCB. There should always be a nearby reference (ground) via. A chip will sense the differential voltage between the signal and local ground. This will be the same voltage that was driven into the trace at the other end of the line, if we have done a good job of maintaining a controlled impedance environment (50 ohms) for the whole length of the trace. The voltage that went in on one end is the same as the voltage that comes out on the other end a time delay later, each WRT to their local grounds. (For the moment, let's ignore the lossy nature of transmission lines.) Now suppose we had a way to measure the voltage between two ground points spaced several inches apart horizontally (I am not sure how to do it, but let's say we could). Suppose there were several volts difference between the two local ground points. Would that make any difference to the waveform propagating on the 50 Ohm transmission line? I don't think so. What ever voltage went into the transmission line WRT it's local ground will come out of the transmission line WRT local ground, even if the local grounds are several volts apart. The driving chip drives WRT local ground and the receiving chip receives a signal WRT local ground. If there happens to be a bunch noisy digital lines on the opposite side of a ground plane, ...so what? BTW, I agree with you that low frequency can be a killer. But signals behave well at high frequency. The thickness of a ground plane is all you need to isolate one signal from another. regards, Larry Smith Sun Microsystems > Date: Wed, 26 Sep 2001 12:27:38 -0700 > From: Zhiping Yang <zhiping@xxxxxxxxx> > X-Accept-Language: en > MIME-Version: 1.0 > To: ldsmith@xxxxxxxxxxxxxxxxxx > CC: si-list@xxxxxxxxxxxxx, james.f.peterson@xxxxxxxxxxxxx > Subject: Re: [SI-LIST] Re: return currents > > Larry, > > What you said about the current distribution at high frequency(>100Mhz) > is true, but my questions is whether the current distribution is important > or the voltage variation on the power plane is more important than current > distribution? > > Let's say, there are 2 points on the power plane and the most (>93%) current > flows > on the surface near digital circuit. The current flow near analog circuit is > very small (<7%), but it has big loop (large inductance) and it produces same > voltage drop between those 2 points as large current on the surface of digital > circuit. > IF the anolg circuit is sensitive to the voltage noise, then it is a problem. > > Jim, another thing you need to be aware is that low frequency may be a killer > for your anolog circuit. In your current stack up, it is diffcult for to > control > the lower frequency current return path on layer 4. > > Thanks. > > Zhiping > > > -- > Zhiping Yang, Ph. D. > Hardware Engineer > Cisco Systems > 270 West Tasman Drive > Mail Stop:SJCG/2/2 > San Jose, CA 95134 | | > email: zhiping@xxxxxxxxx :|: :|: > Tel : 408 525 5690 :|||: :|||: > Fax : 408 526 5504 .:|||||||:..:|||||||:. > ***************************************************** > > Larry Smith wrote: > > > Jim - I don't believe that the high frequency return currents on your > > digital traces will have much effect on your analog traces even though > > they share the same ground plane (layer 4). > > > > The skin depth at 100 MHz is about 0.26 mil compared with the 0.7 mil > > thickness of half oz copper. The skin depth is essentially the depth > > that the magnetic field penetrates into the copper. At 100 MHz, very > > little magnetic field (approximately 1/[e^(.7/.26)] = 7% ) will > > penetrate through the copper plane. Even less of it will reach an > > analog trace. At higher frequencies, the penetration will be even less. > > > > How sensitive are your analog signals? For digital signals, I would > > not worry about 7% magnetic field penetration. > > > > regards, > > Larry Smith > > Sun Microsystems. > > > > > Delivered-To: si-list@xxxxxxxxxxxxxx > > > From: "Peterson, James F (FL51)" <james.f.peterson@xxxxxxxxxxxxx> > > > To: si-list@xxxxxxxxxxxxx > > > Subject: [SI-LIST] return currents > > > Date: Wed, 26 Sep 2001 07:32:10 -0400 > > > MIME-Version: 1.0 > > > Content-Transfer-Encoding: 8bit > > > X-archive-position: 946 > > > X-listar-version: Listar v1.0.0 > > > X-original-sender: james.f.peterson@xxxxxxxxxxxxx > > > X-list: si-list > > > > > > > > > hello, > > > > > > Stackup : > > > > > > 1 - gnd > > > 2 - digital sig > > > 3 - digital sig > > > 4 - gnd > > > 5 - analog sig > > > 6 - analog sig > > > 7 - gnd > > > 8,9,10,11 ..... > > > > > > notice that the digital signals from layer 3 and the analog signals from > > > layer 5 will probably have return currents on layer 4. > > > > > > question : > > > will the digital return currents cause noise in the analog section, since > > > they both share layer 4 for return currents? (My first guess is yes, but > > > someone mentioned that the skin depth for the return currents is small so > > > they can share layer 4 without effecting each other.) > > > > > > thanks for your input. > > > Jim > > > ------------------------------------------------------------------ > > > 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 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 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 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