Ken, Here is my 2c. on it: 2] Evenif the skin dept is smaller, the signals can travel on the plane and can radiate from the edge of the board. It need not be necessarily from the top surface. If you use ground guard band at the edge of the board or use shorting vias at the edge of the board, you can reduce the radiation from theedges. However, the noise signal will get reflected and may interfere withthe wanted signals. Also, it may get into the PDS structure and get coupled to different elements in the PDS (like vias) and get radiated from there. Therefore, it is important to eliminate these signals at the source. 1] It will depend on where and how the ground plane is added. If you add a ground plane so as to make power and ground coupling more tight (and reduce the P/G impedance), then it will be helpful. If your existing ground plane isnearer to the power plane than the new ground plane, then the same phenominon of edge radiation exists. Thanks and regards, Vishram >From: Ken Hayden >Reply-To: khayden@xxxxxxxxxxxxxxxxxx >To: "Grasso, Charles" >CC: "'si-list@xxxxxxxxxxxxx'" >Subject: [SI-LIST] Re: Traces don't cause EMI - really? >Date: Fri, 30 Jan 2004 09:56:24 -0500 >>Thanks for reminding me of Dr. Bogatin's presentation, Charles. I read it when >the si-list first pointed it out, and it's a refreshingly clear treatment of the >subject. If I'm not mistaken, the presentation makes the point that EMI >generated by the plane voltage drop (caused by signal return current) will >generally dominate over EMI from the current loop formed by the signal traceand >its return current. As I understand it, the effect of that plane drop would be >to cause the whole plane to take on an RF voltage, possibly with standing waves >(resonances) as discussed elsewhere in this forum. If that's the case, I have >two questions: >1. Wouldn't the net effect of addinganother ground plane outside such a trace >simply be to reduce the ground drop by less than half, as a result of adding a >second parallel return plane (that's coupled to the first plane fairly >closely)? >2. What about skin effect? I understand that at frequencies of interest >(hundreds of MHz and up), the skin depth is only a fraction of the thickness of >the copper plane. This implies that the plane voltage drop induced on the >inside of an outer plane could not "penetrate" to the outside to radiate. By >extension, if an overall outer ground plane was used, there would be no plane >voltage drop detectable on the outside of the plane. (I know this is nonsense, >but I don't know where my logic is failing.) >-Ken >>"Grasso, Charles" wrote: >>>Ken you may be interested in looking at a presentation made by >>Dr Bogatin that addressed this very subjecy. >>you can find it at http://www.ieee.org/rmcemc go to the archives >>and look for the 2003 December meeting. >>>>Cheers >>>>Best Regards >>Charles Grasso >>Senior Compliance Engineer >>Echostar Communications Corp. >>Tel: 303-706-5467 >>Fax: 303-799-6222 >>Cell: 303-204-2974 >>Email: charles.grasso@xxxxxxxxxxxx; >>Email Alternate: chasgrasso@xxxxxxxx >>>>>>-----Original Message----- >>From: Ken Hayden [mailto:khayden@xxxxxxxxxxxxxxxxxx] >>Sent: Friday, January 30, 2004 6:00 AM >>To: MikonCons@xxxxxxx >>Cc: si-list@xxxxxxxxxxxxx >>Subject: [SI-LIST] Re: Traces don't cause EMI - really? >>>>I read this thread last fall with great interest, and I think I learned a >>lot. But I >>have an immediate application about which I'm still confused, and could use >>some help. >>>>This application is for a PCB that will be assembled into a shielded card>>cage >>assembly. This particular PCB will not have any cables leaving the shielded >>enclosure, >>but any number of other PCBs in this 36-card assembly could have cables of >>various >>geometries and filtering characteristics. (This is a telecom/datacom >>application, and >>the PCBs are line cards with numerous flavors of DSL, Ethernet, POTS, and >>digital >>telecom interfaces.) >>>>We have traditionally laid out PCBs for this application with outside >>planes, and >>absolutely everthing with any high-frequency content was run on inside >>signal layers. >>Using this kind of stackup, and taking many of the usual precautions, we >>have had good >>success in building cards that pass FCC class A, and usually class B. >>>>In the current (very quick-turn) project, we will be using an embedded >>microprocessor we >>haven't used before. In the interest of building fullyfunctional boards >>with good >>signal and power integrity as quickly aspossible, we are considering >>directly lifting >>the processor, DDR SDRAM,gigabit GMII, PCI, and HyperTransport artwork >>section from the >>microprocessor vendor's evaluation kit artwork, and incorporating the >>artwork into the >>rest of our design. >>>>It turns out that this evaluation kit is in PCI plug-in board format >>(clearly intended >>to run ina desktop PC), and has the following stackup: >>>>TOP >>GND >>SIG1 >>GND >>PWR >>PWR >>GND >>SIG2 >>GND >>BOT >>>>This is of course a wonderful stackup for power distribution, but it >>requires running >>close to half of the signals on the outside layers, since there are only two >>internal >>signal layers. The evaluation kit runs many of the DDR SDRAM, PCI, and GMII >>traces on >>the top and bottom layers. Only clocks and HyperTransporttraces seem to be >>strictly >>limited to SIG1 and SIG2. >>>>Myquestion is this: Is this kind of layout likely to radiate significantly >>into other >>boards in the enclosure (relative to a board with more layers, having added >>planes >>outside all signal layers), therebyrisking excessive CM currents from the >>cables >>leading from these other boards? As I have mentioned, we have always >>believed that it >>would, and have avoided such a stackup. But I wonder if we've been going >>overboard and >>wasting money on extra layers. >>>>Ken Hayden >>Consulting Engineer >>Integral Access >>>>------------------------------------------------------------------ >>To unsubscribe from si-list: >>si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field >>>>or to administer your membership from a web page, goto: >>//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: >> nbsphttp://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 >> ---------------------------------------------------------------------------- Let the new MSN Premium Internet Software make the most of your high-speed experience.[1] --- Links --- 1 http://g.msn.com/8HMAENUS/2743??PS= ------------------------------------------------------------------ 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