[SI-LIST] : RE: [SI-LIST] The correct way to short tow nodes in SPICE is?

About this list Date view Thread view Subject view Author view

From: Michael Khusid (mkhusid@sitaranetworks.com)
Date: Fri Oct 20 2000 - 09:24:24 PDT


From reading SPICE manuals some time ago, I vaguely recall description of
using voltage sources in AC simulation. As far as I understood, Spice would
replace all non-AC voltage sources with open circuits. In such a case, a
model with 0 volt Voltage source would also become an open and would cause a
serious error for AC analysis.

Am I right or wrong?

Mike Khusid
Signal Integrity
Sitara Networks
 

> -----Original Message-----
> From: Kim Helliwell [mailto:khelliwe@acuson.com]
> Sent: Friday, October 20, 2000 11:39 AM
> To: si-list@silab.Eng.Sun.COM
> Subject: [Fwd: Re: [SI-LIST] : The correct way to short tow nodes in
> SPICE is?]
>
>
>
> Bo wrote:
> >
> > Hi
> > I would like to discuss one of the big SPICE myths. I have
> used several
> > different spice programs (PSPICE, HSPICE, etc) and I have
> seen two different
> > implementations. The problem is that nobody can agree
> which is the better
> > implementation of the two. I would like to hear your
> opinion on this.
> > The two implementations are:
> >
> > 1) Connect two nodes to each other by putting 0 Ohm resistor.
> > 2) Connect two nodes to each other by putting 0 volt DC
> source between them.
> >
> > Method 1 typically results in resistance set to some small
> value other than 0
> > (by default HSPICE will set it to 1e-5; this can be changed
> in Hspice). I have
> > trying to convince people using this method to at least put
> several of
> > resistors in parallel(just in case someone changed default
> values; in HSPICE
> > this is easily done my setting multipler M to some high value).
> >
> > What is your opinion on this?
> >
> > Regards,
> > Bo
> >
> > __________________________________________________
> > Do You Yahoo!?
> > Yahoo! Messenger - Talk while you surf! It's FREE.
> > http://im.yahoo.com/
> >
> > **** 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
> > ****
>
> I have supported various versions of SPICE for more years
> than I care to
> mention, and, except in Spectre, I *DO NOT* recommend using
> 0-ohm resistors.
> The correct way to model a short is a voltage source of 0 volts. The
> reason for this is that 0-ohm (or very small resistors) will introduce
> a large diagonal element in the matrix representing the
> circuit, which can
> cause large roundoff errors during the solution. This is not
> a good thing
> to do. It can cause inaccuracy of your solution or even
> nonconvergence.
>
> The reason Spectre is different in this regard is that, for
> small resistances
> (including 0 ohms), the simulator uses a branch form for
> modeling the resistor,
> which (guess what?) is exactly the same as putting in a
> 0-volt voltage source.
> So in Spectre, you have a choice, but the end result is the same.
>
> --
> 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
> 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
> ****
>

**** 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 : Tue May 08 2001 - 14:29:48 PDT