Re: gEDA-user: Spice noise analysis

[John Doty <jpd@xxxxxxxxxxxxx>]

As I said, the output is in units of V^2/Hz. It's not in volts, despite
what SPICE claims. If you want volts, you have to integrate over some
passband and take the square root.

John Doty          "You can't confuse me, that's my job."
MIT-related mail:                       jpd@xxxxxxxxxxxxx
Other mail:                             jpd@xxxxxxxxxxxxx

On Sun, 7 Aug 2005, Harold D. Skank wrote:

> Thank you for your advice.  I did get your procedure to work, though I'm
> somewhat in doubt as to how to interpret the results.  Basically the
> onoise_spectrum had about the shape I expected, but the flat central
> region was about 130 femptoVolts whereas the data sheet listed something
> like 2 to 3 nanovolts noise (at the input).  What about this?
> 
> 	Harold Skank
> 
> On Thu, 2005-08-04 at 22:31 -0400, John Doty wrote:
> > In ngspice/tclspice use something like:
> > 
> > noise v(vout) v3 dec 1 100k 10meg 1
> > 
> > v(out) is the point for output noise assesment
> > v3 is the source relative to which input noise is calculated
> > dec means do it by decades
> > 1 means one point per decade
> > 100k means start at 100 kHz
> > 10meg means end at 10 MHz
> > 1 means record source contibutions at each point
> > 
> > Then do "print all": that'll tell you the values, in
> > V^2/Hz. inoise_spectrum is the total input referred noise, onoise_spectrum
> > is the total output referred noise, and the other onoise* are the noise
> > contributions broken down by elementary component and physical noise
> > source. To get the total from a subcircuit, you need to add up all its
> > component noise contributions, or (probably easier here) subtract
> > contributions from components you aren't assessing. It may also be useful
> > to set resistor temps to zero for resistors whose noise you don't want to
> > assess.
> > 
> > To just plot input or output noise, leave out the last argument, and throw
> > in more points:
> > 
> > noise v(vout) v3 dec 10 100k 10meg
> > 
> > Then you'll only get inoise_spectrum and onoise_spectrum.
> > 
> > Beware that this is linear analysis around your DC operating point.
> > Dynamic noise sources associated with changing operating points are not
> > evaluated. You can get some of these by careful use of initial conditions
> > to evalate noise at particular operating points (say, if your Shottkys
> > turn on at some particular phase of input signal and make shot noise), but
> > you'll have to then assess the system effect of such modulated noise by
> > other means. SPICE can't handle things like clock jitter and capacitor
> > switching ("kTC") noise at all, so in general SPICE noise analysis is only
> > part of a total noise assessment.
> > 
> > John Doty          "You can't confuse me, that's my job."
> > MIT-related mail:                       jpd@xxxxxxxxxxxxx
> > Other mail:                             jpd@xxxxxxxxxxxxx
> > 
> > On Thu, 4 Aug 2005, Harold D. Skank wrote:
> > 
> > > People,
> > > 
> > > Attached below is the SPICE file for an Analog Devices amplifier with a
> > > pair of crossed Shottky diodes in front for amplifier protection.  I
> > > need to run an noise analysis to assess the noise contribution from the
> > > Analog Devices amplifier.  How do I do this?
> > > 
> > > 	Harold Skank
> > > 
> > 
>