From: Chan, Michael (Michael.Chan@compaq.com)
Date: Thu Oct 28 1999 - 14:44:04 PDT
I believe that is not what Lee R. intends to say in his original
article. If you have two identical signal traces and each of them has a
signal to ground impedance of 50 ohms and if they are placed far apart so
mutual coupling is negligible, then the differential impedance of this pair
of signal traces will be 100 ohms. This is not true if the pair of signal
are very close together a 100 differential impedance will not necessary
the signal to ground impedance is 50 ohms. You can easily go through the
verify this. This explanation assumes that you don't care about common-mode
current on the common ground; the net current on the common ground of a far
pair of signals may not be zero if the pair is running differentially.
if this is not true.
From: Scott McMorrow [mailto:email@example.com]
Sent: Thursday, October 28, 1999 3:22 PM
Subject: Re: [SI-LIST] : Comments from your SI seminar (SendII)`
The answer is ... "it depends on what you are trying to do."
If you are connecting circuits which are totally contained
within your own system where the design parameters are under
your own control, then all that matters is the timing, skew and
voltage margins at the receivers. If you can prove to yourself
through measurement and simulation that the differential
impedance does not have to be matched and that there is
ample margin for your system, then by all means use the
advise of the article.
However, if your design is close to margins, and/or your design
interfaces to the outside world, then things such as maximum
power transfer, insertion loss, VSWR, and reflections coefficients
come into play.
Basically, for a two wire line, whether it is composed of PCB traces
or twisted pair, the differential impedance is defined to
2 * (self impedance - mutual impedance)
In a Maxwell Matrix this is:
2 * (Z11 - Z12)
Z11 is effectively the characteristic impedance of the line as it is
influenced by all conductors in it's vicinity, including the reference
plane and adjacent traces.
Z12 is the mutual impedance as seen between the two traces in
On a typical PCB with edge coupled traces, the ratio of Z12/Z11
can be as high as 10 to 15%, depending on the spacing of
the two traces. This causes a decrease in the differential impedance.
Two 5 mil traces spaced 5 mils apart which were targeted for
a 50 ohm trace impedance will have a differential impedance
of about 80 to 85 ohms due to the mutual coupling of the traces.
When interfaced to other differential pairs which have a controlled
impedance of 100 ohms, there will be a reflection at the boundary.
This reflection can be measured as VSWR, insertion loss and
attenuation. All of which degrade the performance of the differential
"Denomme, Paul S." wrote:
> I have read an article recently that states that the use of
> specifying the differential impedance of two traces on a circuit board is
> unnecessary. The only thing you need to worry about is the individual
> impedance. If you need a differential impedance for two lines to be 100
> ohms, just use two 50 ohm lines rather than using two signals whose
> differential impedance is 100 ohms. Also when connecting a 110 ohm
> pair to PCB you should just connect it to two 55 ohm traces to achieve the
> 110 ohm differential impedance. I have done enough research to draw my
> conclusions, but I would like to get the reaction from people in this
> regarding this issue.
> Thank you,
> Paul Denomme
> Viasystems Inc.
> > -----Original Message-----
> > From: Doug Brooks [SMTP:firstname.lastname@example.org]
> > Sent: Thursday, October 28, 1999 12:59 PM
> > To: email@example.com
> > Subject: RE: [SI-LIST] : Comments from your SI seminar (SendII)`
> > >But a comment on our industry in general,
> > >
> > > I went to several courses at the PCB Design East, and each course
> > >instructor had their own opinion on what they believe is the correct
> > of
> > >doing things.
> > >It is sad that our industry cannot take a concensus and come up with
> > >CORRECT way of doing things. Instead of using testing and empirical
> > to
> > >determine what is accurate, they bicker about why ones methods will or
> > won't
> > >work.
> > >
> > As a seminar presenter at PCB East, and one who is also concerned about
> > the
> > fact that students hear different things in different courses, I'd like
> > offer a few random comments here.
> > First, people in our industry need a better understanding about
> > fundamental
> > electrical engineering!! And I am not just talking about those without
> > engineering degree, but also those with an engineering degree who (1)
> > didn't take certain kinds of classes related to such high speed issues
> > crosstalk, transmission lines, and stray trace/lead inductance, etc. (2)
> > took them and didn't understand them, or (3) took them and forgot them!!
> > And I am not criticizing them --- in my second job out of college my
> > company was designing state-of-the-art components for the
> > Illiac IV computer that were water cooled ECL devices running at the
> > remarkable speed of 3 MHZ! Things DO change.
> > Second, it's nice to have rules of thumb, but it is better to understand
> > where those rules of thumb came from and when they might (and might not)
> > apply. I often get comments like "In so-and-so's class HE said ...". My
> > response is to try to make the issue UNDERSTANDABLE for the student so
> > he/she can make up his/her OWN mind about what position seems more
> > reasonable. But that can be a challenge when the student has very little
> > technical understanding.
> > Thirdly, as has been pointed out, there aren't a lot of absolutes in our
> > industry. If there were, we'd all understand and be teaching the same
> > (absolute) rules of thumb. While I am a strong supporter of studies (and
> > have contributed to two of them --- the effects of vias on traces and
> > effects of 90 degree corners) this is not always the answer. Because ...
> > each design has a unique environment. So, what works in one environment
> > might not apply to another. Once again, my approach is usually to try to
> > present to the student the ISSUES and the alternative opinions, so they
> > can
> > recognize problems and (hopefully) potential solutions when they arise.
> > before, it is improved understanding that helps the designer (and the
> > engineer) solve problems, not rules of thumb or others' studies.
> > Finally one last observation about studies. We lead a study on right
> > corners where the measurements were taken by the respected people at the
> > University of Missouri (Rolla). The results of that study were
> > independently confirmed by Mark Montrose with (a) a board of his own
> > design
> > and (b) another board from our study. These results have appeared in at
> > least two publications. Nevertheless, take a position on right angle
> > corners in one of these e-mail forums and see how much discussion it
> > generates!! Some people's minds are made up, facts be darned!
> > Doug Brooks
> > .
> > ****************************************************
> > Doug Brooks, President firstname.lastname@example.org
> > UltraCAD Design, Inc. http://www.ultracad.com
> > **** To unsubscribe from si-list: send e-mail to
> > email@example.com. In the BODY of message put: UNSUBSCRIBE
> > si-list, for more help, put HELP. si-list archives are accessible at
> > http://www.qsl.net/wb6tpu/si-list ****
> **** To unsubscribe from si-list: send e-mail to
firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE
si-list, for more help, put HELP. si-list archives are accessible at
-- Scott McMorrow Principal Engineer SiQual, Signal Quality Engineering 18735 SW Boones Ferry Road Tualatin, OR 97062-3090 (503) 885-1231 http://www.siqual.com
**** To unsubscribe from si-list: send e-mail to email@example.com. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****
This archive was generated by hypermail 2b29 : Tue Feb 29 2000 - 11:39:25 PST