From: Joel Amzallag ([email protected])
Date: Mon Mar 26 2001 - 11:02:52 PST
Elias,
One really useful with SPICE simulators option is :
.options opts
it will return you the default options values Spice use and the one you've set.
-Joel.
>Elias,
>In addition to the ones Kim listed, some of my favorite options (but for a
>different spice) to try are:
>.options gmin=1e-9
>.options ABSTOL=1e-9
>.options VNTOL=1e-3
>
>And believe it or not, try a smaller timestep in your .tran statement!
>.tran 10ps 35ns 5ns
>
>Sometimes their isn't enough REAL loss modeled in the circuit and the
>simulator can't resolve the fast changes or noise/ringing.
>
>
>Aubrey Sparkman
>Signal Integrity
>[email protected]
>(512) 723-3592
>
>
> > -----Original Message-----
> > From: Kim Helliwell [mailto:[email protected]]
> > Sent: Monday, March 26, 2001 11:07 AM
> > To: Elias Lozano
> > Cc: [email protected]
> > Subject: Re: [SI-LIST] : internal timestep too small in transient
> > analysis
> >
> >
> > > Elias Lozano wrote:
> > >
> > > I have a question,
> > >
> > > I am having a lot of trouble with this error when doing
> > signal integrity simulations of some I/O buffers with package
> > > models and T models for tranmission lines as well as some
> > loading. I am using HSPICE2000 version. I will change to U
> > > and then W models for more accuracy.
> > >
> > > I would like to get a fresh look at what are the best
> > options to use when having this problem.
> > > In the past, I have had the same problem with TSMC 0.18um
> > models due to some negative-mos conductances?
> > > Is there anyone out there experiencing the same problem and
> > if so any ideas on how to find the right set of options so
> > > that I don't get these erros?
> > >
> > > Once again this is what I am simulating:
> > >
> > >
> > > I/O buffer + Package model + Tmodel + capacitive loading
> > >
> > > I appreciate any comments.
> > >
> > > Regards
> > >
> > > Elias
> >
> > If you are getting TSTS errors with the IBIS buffers, this probably
> > means there is a problem with the buffer model. TSTS errors
> > are mostly
> > associated with MOS models because of the large dynamic range of
> > conductances and the difficulty in insuring that the
> > capacitance models
> > are continuous across the piecewise boundaries. Negative capacitances
> > might do it, too!
> >
> > Here are the steps I would take: I would get in touch with
> > the HSPICE hotline
> > (800.346.5953) and tell them of the difficulties you are
> > experiencing, and
> > get them to take a look at your circuit; they very well may
> > find a bug in
> > the IBIS model code as a result.
> >
> > Meanwhile, the options that help (about 30% of the time) in
> > solving TSTS
> > problems are:
> >
> > Increase ITL4 to 100 (if it isn't already there)
> > Increase RELTOL to .01 (no larger than that!)
> > Set BYPASS=0 (don't allow bypassing)
> >
> > A perusal of Chapter 8 of the HSPICE manual might turn up
> > other options
> > that would help, but the ones above are what I'm familiar
> > with from other
> > simulators. The person answering the phone at the hotline
> > might be able
> > to suggest other options to try.
> >
> >
> > --
> > Kim Helliwell
> > Senior CAE Engineer
> > Acuson Corporation
> > Phone: 650 694 5030 FAX: 650 943 7260
> >
> > **** 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 http://www.qsl.net/wb6tpu
> > ****
> >
> >
>
**** 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 http://www.qsl.net/wb6tpu
****
This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:11:20 PDT