Re: noise question

john larkin <jlarkin_highland_tech> wrote:

On Mon, 15 Jul 2024 19:33:52 +0200, Jeroen Belleman
<jeroen@nospam.please> wrote:
 

On 7/15/24 18:09, john larkin wrote:

On Mon, 15 Jul 2024 17:35:08 +0200, Jeroen Belleman
<jeroen@nospam.please> wrote:
 

On 7/15/24 16:30, john larkin wrote:

Does a negative 50-ohm resistor make as much noise as a regular 50 ohm
resistor?
 
I'd sorta guess the current noise to be the same, and maybe the
open-circuit voltage noise is infinite.
 
I could Spice that, at least the current noise, if Spice handles it
right. LT Spice noise analysis is kind of weird.
 

 
I just tried it: In LTspice the sign doesn't matter,
only the absolute value. Also, if you put a positive
resistor in series with negative one, the noise
voltages add RMS-wise, like you'd expect of independent
sources.

 
Cool. Thanks.
 

 
In real life, a negative resistor may have more or
less noise than an actual resistor, depending on the
low-noise design skills of the designer.
 
I think you knew that...
 
Jeroen Belleman

 
Sure, I was considering an ideal neg resistor, without added noise
from active parts.
 
As a college project, I built a 2-terminal negative resistor and
plugged the negative value into a bunch of equations (voltage
dividers, RCs, LRCs, things like that) and demonstrated that they
worked that way in real life. That was fun.
 
What I was thinking lately was about making an LC oscillator with very
low phase noise, namely low jitter in my world. The finite Q of the
parallel LC is equivalent to a shunt resistor so I'd expect it to have
the Johnson noise of that equivalent resistance. Then the active stuff
must look like a negative resistor, which is noisy too.

 
Yes, that's what I'd expect too.
 

 
LT Spice noise analysis is very limited. I have sometimes added some
random-noise BV blocks in series with resistors and such, so I can do
genuine nonlinear sims with noise. It's actually easier to breadboard.
 

 
BTDT. What's with the nonlinear bit? LTspice noise analysis is
basically an AC analysis, no?
 
Jeroen Belleman

 
LT Spice noise analysis is weird. You need one signal source, even if
you don't use it. And you can only probe one node. It must be entirely
linear.
 
I want to simulate jitter in a LC oscillator, and of course an
oscillator always has some nonlinear amplitude limiting mechanism.
 
 

LTspice has time domain noise sources. They’re actually deterministic, of
course, but you can use a big time offset to fix that.

The scaling iirc 1 sample per second, so you wind up using

noise(1e8*time+2e9)

and stuff like that.

Cheers

Phil Hobbs

--
Dr Philip C D Hobbs  Principal Consultant  ElectroOptical Innovations LLC /
Hobbs ElectroOptics  Optics, Electro-optics, Photonics, Analog Electronics