From: J. Eric Bracken (firstname.lastname@example.org)
Date: Fri Oct 20 2000 - 11:35:34 PDT
> 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 2--using a zero-valued voltage source--is the best way.
The reason has to do with the way Spice handles resistors. It writes a KCL
equation at every circuit node. So if you have a resistor R from node i to node
the contribution of the resistor to KCL at node i is something like this:
vi / R - vj / R
For a zero-valued resistor, 1/R is infinity. The software can't permit this
infinite value to enter into its matrix of equations, so it forces R to some
small minimum value. This minimum value varies from one Spice
implementation to the next.
For a voltage source between nodes i and j, Spice actually writes a
separate KVL equation:
vi - vj = 0
and this is enforced exactly. (At least to the numerical precision of the
matrix solver, which is pretty darn good.)
Only reason I can think of for preferring a small resistor is to avoid
problems caused by loops of voltage sources--which you shouldn't
be creating anyway.
**** To unsubscribe from si-list or si-list-digest: send e-mail to
email@example.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
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:29:49 PDT