RE: [SI-LIST] : How to model effect of vias on nearby traces?

About this list Date view Thread view Subject view Author view

From: Aubrey_Sparkman@Dell.com
Date: Thu Mar 22 2001 - 16:19:20 PST


Larry and Michael,
Can we agree that a trace through any pin field will see either no change,
higher impedance, or lower impedance, all depending on the design of the pad
stack, trace width, and stackup?

Bhavesh,
I would answer that no SPICE including HSpice can determine the impedance of
a trace as it passes through a pin field. For that you need another tool.
To understand the effects of a trace going through a pin field, you need a
two step process. I think that all would agree that since these effects are
geometry (trace width and pad stack design) and material specific, you would
need either a TDR (after design) or a Field Solver to determine the
impedance of the trace as it passes through the pin field.

Only after you determine those impedances can you use your favorite SPICE to
determine the effect of those impedances on your signal. Of course, if your
board is already designed and assembled, you can use a TDR without SPICE to
look at those reflections.

Aubrey Sparkman
Signal Integrity
Aubrey_Sparkman@Dell.com
(512) 723-3592

> -----Original Message-----
> From: Larry Miller [mailto:ldmiller@rhapsodynetworks.com]
> Sent: Thursday, March 22, 2001 4:50 PM
> To: 'Greim, Michael'; Larry Miller; 'Patel, Bhavesh'; SI_LIST (E-mail)
> Subject: RE: [SI-LIST] : How to model effect of vias on nearby traces?
>
>
> Let's say for argument that a trace runs directly over the center of a
> circular antipad area on the reference plane, and the antipad
> diameter is
> larger than the trace width.
>
> Yes, there is no reference under the trace, but wouldn't the
> return paths of
> least inductance go around the rims of the circular antipad?
> That is not a
> much longer path length unless the antipad is huge, so maybe
> that is why
> there does not seem to be much effect.
>
> What seems to really affect things is where you have a gap
> such that the
> return currents have to seek a much longer path length.
>
> Hmmm?
>
> Larry Miller
>
> -----Original Message-----
> From: Greim, Michael [mailto:mgreim@sonusnet.com]
> Sent: Thursday, March 22, 2001 2:40 PM
> To: 'Larry Miller'; 'Patel, Bhavesh'; SI_LIST (E-mail)
> Subject: RE: [SI-LIST] : How to model effect of vias on nearby traces?
>
>
> Wouldn't part of the effect (perhaps a more significant
> part) be how big the antipad is on the reference plane and
> whether the signal in questions is routed over it or not?
> I have seen some antipad requirements so large that a trace
> could be routed over a wafer thin piece of plane to the
> point that the trace is essentially routed over no reference
> at all.
>
> Comments?
>
> Best Regards,
>
> Michael C. Greim Sonus Networks
> mgreim@sonusnet.com 978-589-8336
>
> Making the world safe for digital signals everywhere
>
> And all this science I don't understand
> It's just my job six days a week
>
> The time is gone. The email's over
> Thought I'd something more to say......
>
>
> -----Original Message-----
> From: Larry Miller [mailto:ldmiller@rhapsodynetworks.com]
> Sent: Thursday, March 22, 2001 4:42 PM
> To: 'Patel, Bhavesh'; SI_LIST (E-mail)
> Subject: RE: [SI-LIST] : How to model effect of vias on nearby traces?
>
>
> I have seen some high speed connector TDR plots where traces
> are routed
> through pin fields on back/midplanes. This is similar to
> passing near a via,
> even worse I would think. I have also done TDR's on our own boards.
>
> The effect seems to be very small (a few % of 50 ohms) and of
> short duration
> in time, which of course corresponds to very high frequencies
> (10's of GHz).
>
> One view.
>
> Larry Miller
>
> -----Original Message-----
> From: Patel, Bhavesh [mailto:bpatel@cyras.com]
> Sent: Wednesday, March 21, 2001 8:06 PM
> To: SI_LIST (E-mail)
> Subject: [SI-LIST] : How to model effect of vias on nearby traces?
>
>
> Hi! I wanted to know how do I simulate the effect on the impedance..
> reflection on a trace/signal when it is very close to a via.
> It does not go
> thru the via but passes very close to it. Can I model this in
> HSPICE? And if
> yes how/
> Thanks in advance
> Bhavesh
>
> **** 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
> ****
>
> **** 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
> ****
>
> **** 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
> ****
>
>



**** 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 : Thu Jun 21 2001 - 10:11:18 PDT