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

About this list Date view Thread view Subject view Author view

From: Matt Kaufmann (matt@silicon-spice.com)
Date: Mon Jul 17 2000 - 10:12:02 PDT


RE: [SI-LIST] : inductance extracted by ansoft SI3DDoes 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).
Matt

-----Original Message-----
From: owner-si-list@silab.eng.sun.com
[mailto:owner-si-list@silab.eng.sun.com]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

  Hello:

  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.

  Thanks,

  ===================
  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)
  http://www.tdasystems.com
  The Interconnect Modeling Company(TM)

    ----- Original Message -----
    From: Hassan Ali
    To: si-list
    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
because
> 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 tools?

    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?

    Regards.

    Hassan.

**** 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 - 10:50:47 PST