[SI-LIST] Re: Convergence problem after inserting detailed connector model

  • From: "Ingraham, Andrew" <a.ingraham@xxxxxxxx>
  • To: <si-list@xxxxxxxxxxxxx>
  • Date: Fri, 20 Feb 2004 09:26:53 -0500

Jon wrote:

> I often wonder if anyone from Synopsis bothers to monitor this list. I
> don't
> recall ever
> seeing any advice from them, ...

Actually, I'm fairly certain I have recognized one or two names responding
to mail on this list who are in HSPICE support and have been since before
Synopsis took over.

I wouldn't blame them if they don't advertise that fact, as they could get
inundated with e-mails from everyone on this list who uses it and has ever
had a problem.  After all, their job is to support a commercial product,
through proper support channels, not necessarily to offer free advice to
everyone on this list.

Julia, re: "internal timestep too small" messages:

This is one of the most common and perplexing errors in SPICE, and it
pre-dates HSPICE.  There is no one cause, nor is there one "fix".

Start to get more adventurous with the .OPTIONs.  Try loosening up the
various *TOL options (some of which go by different alias names in Hspice).
Open them up by several orders of magnitude, and if this lets your
simulations work, then go back and tighten them up.  They WILL cause
bogus and misleading results if left very loose.

You've already tried Gear.  Things that work for one person's circuit, may
do nothing in another's.

Component values spanning a very wide range tend to not do well in Spice.
So if you have micro or milliohm and megohm resistors in the same
simulation, see whether you really need the tiny ones.  If someone added
tiny resistors to make "connections" between nodes, replace them with shorts
or 0V voltage sources.  This may go against your conscience or your gut
feelings, but lots of 0V voltage sources are usually much better in Spice
than lots of 1e-6 resistors are!

There are Hspice options that will add a small capacitor, or a small
conductance, at every node, not just a few.  Try playing with these too if
you haven't already.  Don't be afraid to use values much larger than
actually exist.  Your first job is to get the darned thing to converge; then
you can go back and tweak things until it just doesn't break.

Try simulating the connector model and everything else separately, as a
sanity check.  Or try different drivers and receivers with the connector
model.  Alas, many Spice problems don't show up until you connect things
together, as if the elements are somehow "incompatible" in some way.

If it is a complex connector model, maybe there is something wrong, either
with the model or how you are using it, so make sure to try it with
different connections (terminated or open or short circuited on the various
pins) to see if one of them causes ill behavior.

There could be issues with grounds on the two sides of the connector model;
make sure you fully understand how it is supposed to be used in that regard.
If node 0 appears on both sides, might that be an unrealistic sneak path
short-circuit around the connector?  Some models are meant to be used that
way, some aren't, and some models probably don't handle grounds right
anyway.

Regards,
Andy


------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List technical documents are available at:
                http://www.si-list.org

List archives are viewable at:     
                //www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu
  

Other related posts: