Thanks for sharing! This ("a 100-Ohm trace radiated >6 dB more than a 50-Ohm trace") seems = to agree with Dockey's paper - the farther away you are from the = reference plane (and, consequently, the higher the impedance), the more = EMI you radiate. The question I'm confronted with at this point is: do "well-behaved" = single-ended signals generate appreciable EMI? Dockey's paper outlined = the effect, but with geometries (90mil wide trace over a 62mil = dielectric) that aren't likely to be used. He then demonstrated the = reduction in EMI when the trace was brought closer to the reference = plane. Given current geometries, is it likely for a bus of properly = designed single-ended traces to cause failing EMI? My = experience/impression is no. =20 If that's incorrect, please let me know. On the other hand, as I understand it, differential traces are much more = "forgiving", EMI-wise, of non-idealities. And these we often induce, = knowingly or not. So, tightly-coupled differential traces are = desireable, EMI-wise, given our imperfect world and the issues we must = deal with. That's not to say there aren't other reasons, besides EMI (increased = loss, and some yet to be discovered/published), why we may NOT want to = route differential traces closely-coupled. Unless I'm incorrect about current single-ended traces and their = tendency (or lack of) to generate EMI, I'd stick with my original = assertion, that closely coupling differential signals has benefits, but = is not absolutely necessary for their entire length (but compensation = for impedance change due to reducing or increasing coupling might be = necessary). Thanks for your time/energy. Actually, I've been contracted by the = fishees to distract you from pursuing them :-) Jeff Loyer -----Original Message----- From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of MikonCons@xxxxxxx Sent: Thursday, October 16, 2003 11:33 AM To: si-list@xxxxxxxxxxxxx Subject: [SI-LIST] Re: Traces don't cause EMI - really? In a message dated 10/16/2003 10:14:54 AM Pacific Standard Time,=20 jeff.loyer@xxxxxxxxx writes: Just to be clear - are you saying that if I connected 2 properly = designed=20 chips (driver and receiver) together with many properly designed = single-ended=20 transmission lines, they would likely fail FCC standards? Yes, but only with qualifications. Picture a single-ended, 50-Ohm = microstrip,=20 not multiple closely spaced traces. If excited with a 1 ns risetime = signal at=20 33 MHz clock frequency from a 50-Ohm generator, and terminated with a = 50-Ohm=20 chip resistor, expect failure. For example, the EMCAD1 software = application=20 (circa 1992) is based on radiated emissions equations and predicts ~39 = dBuV at=20 33 MHz at 30 meters antenna distance. The first few harmonics are also=20 predicted to be out of limits. Note that this software uses worst-case = predictions.=20 The same software also indicates an increase in the single-trace = emission level=20 by SQRT(N), where N =3D the number of traces; however, the assumption is = that=20 all traces are carrying the same excitation (which is unrealistic).=20 Now, if you place grounded planar areas around the trace, or have a = densely=20 routed board, the additional copper provides a substantial reduction in = the=20 measured emissions from that single trace because many field lines that = would=20 otherwise leave the board terminate on the added copper (even though = they may be=20 additional 50-Ohm traces). And, in a normal board design, many of the = signals=20 on these surface traces will generate fields that cancel each other.=20 Therefore, the bare (i.e., unshielded, and unenclosed) PCB MAY or MAY = NOT fail an FCC=20 or CISPR radiated emissions test.=20 The IBM paper I mentioned recorded up to 20 dB variation in radiated=20 emissions from a single microstrip on a bare board as the trace was = moved in-board=20 from the PCB edge. This measured reduction also illustrates the = field-capturing=20 effect of surrounding copper, reference planes, or other conductors. The PCB I created contained significant open surface space around the = traces=20 (including the guarded trace structures) which tended to increase the = radiated=20 emissions relative to a real board design, but this was on purpose to=20 illustrate the effect. As an added note, I found that the radiated emissions from a single = trace=20 increased more than linearly with the impedance of the line; i.e., a = 100-Ohm=20 trace radiated >6 dB more than a 50-Ohm trace. This result makes sense = as a better=20 match to the 120*pi =3D 377 Ohms of free space is achieved with the = 100-Ohm=20 line. Mike Michael L. Conn Owner/Principal Consultant Mikon Consulting *** Serving Your Needs with Technical Excellence *** ------------------------------------------------------------------ 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: =20 //www.freelists.org/archives/si-list or at our remote archives: http://groups.yahoo.com/group/si-list/messages=20 Old (prior to June 6, 2001) list archives are viewable at: http://www.qsl.net/wb6tpu =20 ------------------------------------------------------------------ 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