Current of Spectre simulation

[Xintian Shi]

Hello,

I have a question about the Spectre simulation in Cadence analog design
environment.
-- I ran a simulation and watched the currents in some nodes. The strange
thing is that the sum of current at a node is not zero (doesn't fullfil
Kirhoff's law). e.g. Two transistors are connected in serial, but the
currents of the 2 transistors are not equal. Is it possible?
Anybody could give me an explanation?
Thanks for help.

 

[Svenn Are Bjerkem]

In article <437368fc$0$1151$5402220f@news.sunrise.ch>,
xintian.shi@unine.ch says...

Two transistors are connected in serial, but the
currents of the 2 transistors are not equal.

Do you have bulk contacts? Any current there?

--
Svenn

 

[Andrew Beckett]

On Fri, 11 Nov 2005 08:07:07 +0100, Svenn Are Bjerkem <svenn.are@bjerkem.de>
wrote:

In article <437368fc$0$1151$5402220f@news.sunrise.ch>,
xintian.shi@unine.ch says...
Two transistors are connected in serial, but the
currents of the 2 transistors are not equal.

Do you have bulk contacts? Any current there?

Also, you have to be aware that the gmin conductances added for convergence
(normally 1e-12 mho) also draw some current...

Other explanations can be that you have the devices implemented as inline
subckts, where there is more than one component connected to the pin. WIth
inline subckts, the current reported is the current through the inline device,
not the whole subckt.

Another problem can be that there have been bugs in the past where the current
reporting was incorrect (it was solved correctly, but reported wrongly) with
some device types. However, I believe all these issues have been resolved
now (the most recent I'm aware of was the current through the bulk pin of a
bsim4, if I remember rightly). Check to see if setting "useprobes=yes" (via the
Save All form in ADE) fixes it (this tells spectre to always measure currents by
putting an iprobe in series rather than using the built-in current output of the
device).

Regards,

Andrew.