Re: [SI-LIST] : Trace Impedance Selection

About this list Date view Thread view Subject view Author view

From: Scott McMorrow (scott@vasthorizons.com)
Date: Thu May 04 2000 - 19:11:21 PDT


Doug,

My responses are below.

best regards,

scott

--
Scott McMorrow
Principal Engineer
SiQual, Signal Quality Engineering
18735 SW Boones Ferry Road
Tualatin, OR  97062-3090
(503) 885-1231
http://www.siqual.com

Doug Brooks wrote:

> Scott, > > Many good points, thanks. > > But see two questions: > > >A lower Z0 causes greater mismatch to long package stub sections > >on multidrop > >lines and can accentuate resonance effects at high edge rates. > > Would you expand a little on this one?

Aahh ... on a multidrop bus a package stub sees two trace sections on insertion into the board at the pin. Thus, the characteristic impedance that a device sees when looking out from the die and into the board is Z0/2. Many packages have fairly long internal stub lengths approaching significant fractions of a rise and fall time. As such, the package is itself a transmission line and commonly has an impedance in the 40 to 70 ohm range. As we lower the PC board trace impedance the mismatch at the pin/board boundary becomes larger. As the PCB trace impedance on a multidrop net is reduced, more energy is reflected back towards the die. Since the die is essentially an open circuit we form a very nice 1/4 wave resonator. Although the Q of the resonator is rather low, due to loss effects in the package and die, there is still enough resonance occuring to cause some very interesting effects on high speed busses ... especially at data rates beyond 1 GHz.

> > > >I lower Z0 trace will generally have lower coupling to neighboring > >nets. > > Why? (i assume you are talking about cross talk, here)

Yes, if we fix the trace to plane spacing, then impedance would be controlled by trace width. In the low impedance case there are more field lines in contact with the plane, and the center of the current distribution is further away from other traces on the board. (I am, of course, assuming that the edge to edge trace spacing also remains constant.)

If trace to plane spacing is used to lower impedance, rather than trace width, then the benefit for crosstalk is even more pronounced, since there is even tighter coupling to the neighboring plane.

> > Thanks > > Doug > > .

**** To unsubscribe from si-list or si-list-digest: send e-mail to majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu ****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Wed Nov 22 2000 - 10:50:11 PST