RE: [SI-LIST] : inductance extracted by ansoft SI3D

About this list Date view Thread view Subject view Author view

From: Farrokh Mottahedin ([email protected])
Date: Mon Jul 17 2000 - 10:58:16 PDT


TDRs can and have been used to isolate and quantify the effects of vias.
You may be interested in reading an excellent article tiltled "How Do Vias
Affect High-Speed Circuits?" by Lee Ritchey in this month's (July 2000)
issue of Printed Circuit Design.

Farrokh Mottahedin

Quantum Corp.
500 McCarthy Blvd.
Milpitas, CA 95035
[email protected]

-----Original Message-----
From: Matt Kaufmann [mailto:[email protected]]
Sent: Monday, July 17, 2000 10:12 AM
To: si-list
Subject: RE: [SI-LIST] : inductance extracted by ansoft SI3D

Does TDR have enough resolution to isolate the effects of a single package
via (maybe only 0.1-0.3mm long) from other elements (traces, other vias) in
the package? My understanding is that TDR resolution is on the order of 1-2
mm (after converting time to distance).


-----Original Message-----
From: [email protected]
[mailto:[email protected]]On Behalf Of Dima Smolyansky
Sent: Monday, July 17, 2000 9:35 AM
To: si-list
Subject: Re: [SI-LIST] : inductance extracted by ansoft SI3D

There is always, of course, the way of the TDR.
If the via is so long compared to system rise time that it needs to be
considered a distributed elements, TDR extracts the Z and Td quite nicely.
If it is necessary to compute L and C of the via separately, extending the
JEDEC publication JEP-123 from packages to other elements, one can do it, as
long as one is able to create appropriate test structures beforehand. R is a
separate issue, but R is typically a small number, millohm one hopes, is it
not? In that case, it is best measured with a DC meter, which can provide an
accurate value.
There are also TDR techniques for computing partial or loop inductance
values, depending which is required.
Dima Smolyansky
TDA Systems, Inc.
11140 SW Barbur Blvd., Suite 100
Portland, OR 97219
(503) 246-2272
(503) 246-2282 (fax)
(503) 804-7171 (mobile) <>
The Interconnect Modeling Company(TM)

----- Original Message -----
From: Hassan Ali <mailto:[email protected]>
To: si-list <mailto:[email protected]>
Sent: Monday, July 17, 2000 7:47 AM
Subject: RE: [SI-LIST] : inductance extracted by ansoft SI3D

> > 2.For a via through several power and ground planes, does the SI 3D
> > consider the effects of those planes when doing the extraction?
> >
> For this I believe you need a full wave solver such as their HFSS. Edge
> rate (frequency content) & geometry really are the factors. If you edge
> rate is slow compared to the geometry, then the complication of an
> additional solver MAY not be necessary. But, since we MAY not know all
> those rules of thumb & guidelines, take no chances & use a full wave
> you probably do have edge rates which are "fast". Your investment in
> understanding a refined full wave solver will be worth it.

As to the original question, AFAIK (as far as I know) Ansoft SI Q3D is NOT
capable of computing via parasitics in consideration to individual planes.
You see, SI Q3D considers the entire via structure comprising of the signal
traces connected to the via, the via barrel (the plating on the via hole),
and all the pads at different layers, as ONE conductor. ALL the ground
planes are considered connected hence they make ONE conductor. In that case,
the self L and R values computed for the via structure are for the ENTIRE
via structure as mentioned above (i.e. not just for the via barrel), and the
capacitance to ground is with reference to ALL the ground planes (i.e. you
don't get separate values for capacitance with reference to EACH individual
ground plane). That information is not very useful for critical SI analysis.
And unfortunately, I don't know of any software tool that can accurately
compute separate parasitics. Any suggestions?

To illustrate further the problem in question, suppose I want to include via
parasitics for a signal that goes from the top pcb layer to an inner signal
layer, then I need to include via parasitics of only that portion of the via
that gets into the path of my signal i.e. not the parasitics of the entire
via structure. Any body knows how to do that with the presently available

As to the capabilities of HFSS, I think many people make wrong assumptions
on how full-wave field solvers can help us (SI engineers). First of all HFSS
would NOT spit out via parasitics! Using your various signal traces as
"ports", HFSS can accurately compute scattering (S) parameter matrix for all
the ports. These S-parameters are computed for each propagation mode of
interest (e.g. TEM mode) and indeed takes into account the electromagnetic
(EM) field interactions of all the structures in the geometry of the problem
(e.g. for a via, all the conductors, power and ground planes).

That is well and good, but the problem is that you CANNOT (easily) separate
individual interactions in terms of R, L, and C parasitics. The only method
I know of is to find a lumped-element equivalent circuit (which may not be
unique) and use a microwave circuit simulator (like Touchstone, Libra, ADS,
MDS, Ensemble, SuperCompact, APLAC, etc.) to optimize the R, L, and C,
values to make the equivalent circuit have the same S-parameters as the
original 3D structure. This is a painful process and at best not accurate
and reliable. This is because, at high frequencies, all the parasitics are
distributed and therefore cannot (easily) have an accurate lumped-element
equivalent. Am I too much of a pessimist here? Any ideas of what works best?



**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected] 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

About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Wed Nov 22 2000 - 10:50:47 PST