[SI-LIST] Re: Convergence problems with Hspice

Hi Khalid,
Use the .Options Converge=1, 2, 3 which uses different methods to
converge the simulation. It will give you more details on the problems
with the simulations. Also, if you haven't tried it yet, set the
.options Method=Gear which uses a different integration method for
transient solution (by default HSPICE uses a Trapezoidal method of
integration). 

Look in the manual for further details. Look at the listing of non
convergent nodes in the output file to see which ones have the highest
error, and work backward from there. Most times by looking at this you
can isolate which component is giving you the problem. 

One thing I have found is that most times convergence problems are
present there tend to be either  discontinuities in the IC models,
things are not properly connected, or small segments of t-line/w-line. 

Is your convergence condition "timestep too small" or is it a DC
convergence problem? If it is a DC convergence problem, you can probably
adjust GMINDC to (no more than) 1e-9, I think default is 1e-15. If it is
a timestep problem, look for small segments of transmission line (or
w-line) (<200mils or <10mm) they may be in your package model, if these
are used you can probably get away with substituting a 0.01 ohm resistor
and add the approximate delay to your results (if this matters to you).
Lastly it may be benneficial, if you have inductors in your simulation,
to connect a resistor 1Meg in parallel to achieve convergence.

These are the initial steps I would take. 

I hope this helps,
Peter

Khalid Ansari wrote:
> 
> Hi,
> 
> I am trying to run some spice simulations but running into problems.  What
>   I have is three blocks, basically, a driver, the package model for the IC
> and
> 30 inches of trace (created using the W transmission line model).  When I
> run the driver by itself it looks like it is supposed to.  Driver + package
> model
> looks good.  Driver + transmission line model looks good, but when I put all
> three together I run into all kinds of convergence problems.  The package
> models
> were created using Ansoft Spicelink, the version of hspice that I am using
> to run
> these simulations is 2001.2.  Has anybody seen similar errors trying to run
> simulations which are similar to mine.
> 
> Thanks in advance,
> Khalid
> 
> ------------------------------------------------------------------
> 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:
> http://www.freelists.org/webpage/si-list
> 
> For help:
> si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
> 
> List archives are viewable at:
>                 http://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
> 

-- 
Peter LaFlamme

Applied Micro Circuits Corp.
Staff System Applications Engineer
200 Minuteman Rd, 3rd Floor
Andover, MA 01810

978-247-8470 phone
978-623-0055 Fax
------------------------------------------------------------------
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:
http://www.freelists.org/webpage/si-list

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

List archives are viewable at:     
                http://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: