The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> SPICE syntax re: differential noise evaluation
https://designers-guide.org/forum/YaBB.pl?num=1213718168

Message started by joel on Jun 17^th, 2008, 8:56am

Title: SPICE syntax re: differential noise evaluation
Post by joel on Jun 17^th, 2008, 8:56am

I wonder if you smart people could answer a how-to question for me. I'd like to evaluate the small-signal noise of a differential opamp. The spice manual explains that the .noise statement takes two arguments. The first is the output variable defining the output voltage from which the noise is evaluated. The second is the indepenant source to be used as the noise input reference. So if I want to evaluate the noise at the differential outputs of an opamp with single-ended input, I'd type

.noise v(outp,outn) Vinp

Where outp, outn are the output nodes of the circuit, and Vinp is the independent voltage source defining the voltage of the input node of the circuit, e.g. Vinp inp VCM 0 AC 1 .

This seems to work. But if I want to evaluate the noise of the circuit with a differential input configuration, do you know the syntax? I'd be defining the input like this:

Vinp inp VCM 0 AC 0.5 $inp positive polarity input node
Vinm inm VCM 0 AC 0.5 180 $inm negative polarity input node

My confusion is that I'm now driving the circuit with two independent sources. Maybe it doesn't matter, or I need just do a 6dB adjustment?

I hope my question make sense. Thanks for any knowledge you can offer me!

Title: Re: SPICE syntax differential noise evaluation
Post by Frank Wiedmann on Jun 17^th, 2008, 9:46am

Use the ideal balun from http://www.designers-guide.org/Analysis/diff.pdf and take the voltage source at the differential input as reference.

Title: Re: SPICE syntax differential noise evaluation
Post by joel on Jun 17^th, 2008, 12:42pm

Thanks, that sounds perfect! Please excuse my ignorance and let me ask another question. The balun subckt definintion contains two independent voltage source definitions:

V1 3 5
V2 2 7

These statements seem to specify the source & reference nodes, but not the potential between them. I'm more accustomed to, for example, V1 3 5 0.75V . Could you comment on how these two statements behave in the subckt?

thanks in advance, /jd

Title: Re: SPICE syntax differential noise evaluation
Post by ywguo on Jun 17^th, 2008, 6:58pm

Hi Joel,

Which cell do you use in analogLib? I use ideal_balun. The subckt for it is shown below in spectre language.

Code:

subckt ideal_balun d c p n
K1 ( d 0 c n ) transformer n1 = 2
K0 ( d 0 p c ) transformer n1 = 2
ends ideal_balun

Yawei

Title: Re: SPICE syntax differential noise evaluation
Post by Frank Wiedmann on Jun 17^th, 2008, 11:17pm

joel wrote on Jun 17^th, 2008, 12:42pm:

The voltage across these voltage sources is zero. They are used to measure the current flowing through them and are referenced by the current-contolled current sources (F elements).