[SI-LIST] Re: Big Hspice Netlist Question

Hi Zhangkun,

Do you have large linear network with comparatively small number of
ports?
Or can your design be represented as a connection of several large
linear networks with small number of ports (up to 10-20) and nonlinear
devices? If yes, then you can dramatically increase simulation speed and
accuracy by converting your linear subcircuits into S-parameter models.
This way you perform "model compression": you get rid from huge amount
of linear elements and internal nodes.

I would especially recommend using CPF method in ELDO. With ELDO, you
can define linear multiport and generate Touchstone S-parameter file by
AC analysis. Then, this file can be used to define the S-model instance
when you need time-domain simulation. You do not need to create
equivalent circuit. The algorithm is linear in complexity.

The benefits are the following. Your large linear network shrinks into
condensed S-model, without thousands of RLC elements and internal nodes.
What is even more important, in ELDO, S-model does not perform direct
convolution or numerical integration but uses semi-analytical
computations. Because of that, S-models do not produce LTE (local
truncation error) at all. Because of that, you can select much larger
time step and get more accurate solution. This is especially important
for long time-domain simulations (e.g. if you want to build eye-diagram)
where LTE makes a very bad things.

It is not uncommon that by compressing the large RLC network into
S-model we reduce simulation time from days to an hour, with better
accuracy.

Vladimir


Msg: #4 in digest
Date: Thu, 30 Dec 2004 16:59:15 +0530
From: Vinayak AGRAWAL <vinayak.agrawal@xxxxxx>
Subject: [SI-LIST] Re: Big Hspice Netlist Question

I do not use HSPICE, but I have used eldo, hsim and, to some extent,=20
spectre.

There is an option available in the first two that can do a=20
serial-parallel reduction of all components prior to simulation. I guess

something similar should be available with HSPICE.

Otherwise you need more RAM on your computers (or perhaps change the=20
software).

Vinayaj




Zhangkun wrote:

>Dear Expert
>In my simulation, there is a big HSPICE netlist. When I run it, the
computer tells me that the memory is not enough. Could any expert help
me to solve this problem?
>
>In the netlist, there are 16000 pieces of inductors and 19200 pieces of
resistor. Is it possible to simulate this kind of netlist?
>
>Any advice would be helpful.
>
>Best Regards
>
>Zhangkun
>2004.12.30
>
>

------------------------------------------------------------------
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 FAQ wiki page is located at:
                http://si-list.org/wiki/wiki.pl?Si-List_FAQ

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

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: