Before I started I have to say I am also a big fan of ground via = stitching around edges of PCB. That said. In your experiment, did you provide ground return current = vias near your differential pair transition via ? One can easily design = an experiment where return current path is denied (no ground vias near = the signal vias) and it is forced to return through plane coupling (i.e. = to justify thin core capacitance planes) or your via stitching (to = contain the large EMI radiation field). Neither is the correct solution = to the problem which is lack of return current vias. Another thing to consider is in real live non-backplane PCB's, there are = tens of thousands of ground vias by IC's and passive components = sprinkled around the PCB, it will be hard to find a large piece of = via-less plane to start your resonance. -----Original Message----- From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of pritchard_jason@xxxxxxx Sent: Tuesday, October 30, 2007 10:32 AM To: si-list@xxxxxxxxxxxxx Subject: [SI-LIST] Re: DDR2 2-slot design preference... I contributed to the paper, so I'll try and shed some light on what was in it... The purpose of the paper was to explain how high frequency energy can travel across a PCB and radiate from PCB edges or end up in areas you didn't expect it to be.=3D20 If you spend a little time in the lab taking EMI measurements then you will find out that if you take any board with high speed serial links with via transitions or stripline routing, and measure around the edge of the PCB you will almost always find energy there. The question I always had was, how did it get there? I have been doing SI for many years so I typically thought about problems in 2 dimensions. The problem with EMI is it's 3 dimensional. It is sometimes difficult to predict how energy will travel. The first step is knowing the mechanisms in which energy gets diverted and spread out across the PCB.=3D20 The first thing we did was set-up simple experiments in SI-Wave to try and figure out what was going on. We created simplified etch layouts of the real board that was having problems. We soon came to the conclusion that via transitions were exciting resonances on the PCB. What we determined was that the size of your reference plane and the resultant cavity resonances created between 2 planes caused energy to travel in the direction of the resonances when excited by via transitions. This loss of energy to the planes can also be seen in the s-parameters of the etch. That is essentially the first half of the paper.=3D20 We then went into the lab. The experiments were done on a backplane test board. It only had ground planes. We chose this board because it had SMA connections and allowed us the flexibility to apply whatever input we wanted. It also had the same etch/via structures of our problem board, and proves the point that it doesn't matter if its power or ground. All you need is 2 metal pieces to create a cavity resonator.=3D20 The simulations and lab measurements proved that you could predict where emissions would occur on a PCB. Did this experiment actually solve a real problem? Indirectly. Once we knew what mechanisms allowed energy to go to unwanted places on a PCB you can change the layout to accommodate this. One solution is to use via stitching along the edge of the PCB to reduce the impedance so that it cant radiate. This was implemented because the board slipped into metal clips at the edges of the PCB. If you can squelch the noise before it gets to the metal clips you can reduce the amount of energy directly coupled to the chassis. Another solution would be to make sure your return path impedance is very low along all of your high speed signals which is very difficult in high density boards.=3D20 You could consider via fencing along the edge of a PCB a "rule of thumb", but it's a useful one because I have yet to see anyone capable of looking at a PCB and tell me how the energy is going to travel across the PCB, couple, and radiate. This is not a 2D SI problem its 3D. Obviously you could put the work in and simulate it, but that is often time consuming and not available to most people.=3D20 We were going to present the REAL board results at design con in February but it wasn't in the cards this year.=3D20 I am not an EMI "guru". I just wanted to understand what is happening. Just because you haven't seen it doesn't mean it doesn't exist.=3D20 References:=3D20 * Reducing Simultaneous switching noise and emi on ground/power planes by dissipative edge termination. Istvan * EMI mitigation with multilayer Power Bus Stacks and via stitching of reference planes. Xiaoning ye, David M. Hockanson, Min Li,..... * Radiated Emission from a multilayer PCB with traces placed between power/ground planes. Takashi Harada, Hideki Sasaki, Toshihide Kuriyama * Reduction in radiated emission by symmetrical power-ground layer stack-up pcb no open edge. Satoru Haga, Ken Nakano, Osamu Hashimoto * The Radiation of a rectangular power bus structure at multiple cavity mode resonances. Marco Leone * Coupling of through hole signal via to power/ground references and excitation of edge radiation in multilayer PCB. Jun So Pak, Jingook Kim ..... -Jason This email and any attachments thereto may contain private, = confidential, and privileged material for the sole use of the intended = recipient. Any review, copying, or distribution of this email (or any = attachments) by others is strictly prohibited. If you are not the = intended recipient, please contact the sender immediately and = permanently delete the original and any copies of this email and any = attachments thereto. ------------------------------------------------------------------ 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.net 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