IPC-D-317A, "Design Guidelines for Electronic Packaging Utilizing High-Speed
Techniques" gives equations for microstrip, embedded
microstrip, stripline, and some other transmission lines. The course notes for
Rick Hartley's course "High Speed Design: A Practical
Approach" has these equations along with equations that he got from various
printed circuit board (PCB) fabricators. Rick's suggestion
was to use these equations as a starting point. Then talk with the PCB
fabricator(s) that you want to use, and get them to recommend
trace widths and dielectric thicknesses for your desired impedance. As a
practical measure, he suggested putting one transmission
line of each impedance into a spare area of each card, or in a scrap area of the
panel, that could take an SMA connector. That way the
PCB fabricator could directly measure the impedance-- on your card-- using a
Time-Domain Reflectometer (TDR) for process control.
Doug Brooks, in some of his Brookspeak columns in Printed Circuit Design
magazine, has pointed out that the dielectric constant of
epoxy-glass depends not only on the epoxy-to-glass ratio, but also to the degree
to which the epoxy has been cured. (Thus a smart PCB
fabricator can, on a batch-by-batch basis, juggle the transmission line
impedance to be very close to your desired value despite all the
other variables in the process.) The dielectric constant is also a function of
frequency. Some transmission-line-impedance formulas and
some of Doug's columns are available at http://www.ultracad.com/
John Barnes Advisory
email@example.com on 01/13/99 11:37:50 AM
cc: (bcc: John Barnes/Lex/Lexmark)
Subject: Re: [SI-LIST] : Transmission Lines Formulae
The formulae provided in different reference books are not very accurate,
but are subject to several approximations. It is good to use these
formulae only for obtaining a ball park figure. For greater accuracy, one
should use a 2-D, or 3-D field solver. Again, the PCB building processes
have common tolerances of no better than +/- 10%, unless one is willing to
pay big bucks for tighter tolerances.
The best approach I have found out is to have the PCBs built based on your
calculations/field solver analysis, and then perform an actual impedance
measurement with TDR. The difference between calculated and actual
impedance value is the adjustment you need to make for the PCB
manufacturing process. Hence, it pays to stick with one fab for all your
HyperLynx provides a reasonably accurate 2-D field solver as part of their
Crosstalk analysis tool, and it is very easy to use.
PCB Development and Design Department
IBM Corporation - Storage Systems Division
Always do right. This will gratify some people and astonish the rest.
.... Mark Twain
Lum Wee Mei <firstname.lastname@example.org> on 01/12/99 06:01:00 PM
To: "'email@example.com'" <si-list@silab.Eng.Sun.COM>
cc: (bcc: Ravinder Ajmani/San Jose/IBM)
Subject: [SI-LIST] : Transmission Lines Formulae
While working on my Z calculation for transmission line, I noticed that
different reference books provide different variations of the
transmission line formulae be it microstrip or stipline.
As a designer, I am expected to be proffesional in my work and able to
explain the rationale why I use the formulae from this reference book
and not the other. Can someone enlighten me on which formula to use and
the reason, if any?
BTW, an engineer in another dept of mine mentioned that I need not have
to bother with manual Z calculation because the PNC SI tool is able to
extract the information. I have attended the PNC workshop and do not
find it friendly to use. Moreover, the accuracy of the output depend
heavily on the accuracy of the input. That is just my feeling ;)p, I do
not know about the rest of you who have use this PNC SI tool?
Hope to hear from anyone of you.
Thanks and regards.
**** 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
**** 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 http://www.qsl.net/wb6tpu/si-list ****