The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Unexpected value of noise
https://designers-guide.org/forum/YaBB.pl?num=1276201020

Message started by Vladislav D on Jun 10^th, 2010, 1:16pm

Title: Unexpected value of noise
Post by Vladislav D on Jun 10^th, 2010, 1:16pm

We all know that the output noise of two resistor is 4*k*T*(R1 || R2). So, if both resistors have value of 50 Ohms, the output noise is 0.644nV/sqrt(Hz) (T=300K). If I simulate the circuit with two resistors and a voltage source I get the same result, however, if I substitute series resistor and voltage source with 50-Ohms port the output noise becomes 638nV/sqrt(Hz). I cannot find the explanation of this effect. Is this bug or I missed something?

Title: Re: Unexpected value of noise
Post by rfcooltools.com on Jun 10^th, 2010, 9:56pm

In Cadence the port has its own temperature. you may want to check what the default is set to.

http://rfcooltools.com

Title: Re: Unexpected value of noise
Post by pancho_hideboo on Jun 12^th, 2010, 7:52am

I can't find out any design isuue in your question.
Your question is no more than very easy issue of very specific vendor's simulator.

What simulator do you use ?

Vladislav D wrote on Jun 10^th, 2010, 1:16pm:

if I substitute series resistor and voltage source with 50-Ohms port
the output noise becomes 638nV/sqrt(Hz).

V_out²=4*k*{R₂/(R₁+R₂)}²*(R₁*T₁+R₂*T₂)
Here R₁ and T₁ mean resistance and temperature of "port" respectively.

If R₁=R₂=50, V_out²=50*k*(T₁+T₂)

If T₁=T₂=300K, V_out=643.6[pVrms/sqrt(Hz)].

If T₁=290K, T₂=300K, V_out=638.2[pVrms/sqrt(Hz)].

See http://www.designers-guide.org/Forum/YaBB.pl?num=1192525133/10#10

The followings are general notes for you.

- Always describe correct tool's name and vendor's name which you use as tool or simulator.
- Don't do multiple posts which are same content.
- Don't request source code or behavioral model without any efforts.
- There are many simulators which have analyses called as PSS, PAC and Pnoise.
- Describe in detail with using correct terminologies.
- Warnigns are different from Errors.
- ADS is not name of simulator.
- There is no tool which name is Cadence.
- Don't use Direct Plot of Cadence ADE blindly without knowing definition.
- All gains in Direct Plot of Cadence ADE are "right", "true" and "practical" voltage gain.
- Don't mix up Simulation with Post Processing. They are completely different phase.
- MATLAB are different from Simulink.
- Learn measurements using actual instruments. Not "EDA Tool Play

Title: Re: Unexpected value of noise
Post by pancho_hideboo on Jun 14^th, 2010, 6:07am

Agilent ADSsim treat temperature of port as analysis temperature, if it is not specified for all analyses except for SP-Analysis.
In SP-Analysis of Agilent ADSsim, ADSsim treats port temperature as 290[K] even if you set any value as port temperature.

Again see http://www.designers-guide.org/Forum/YaBB.pl?num=1192525133/10#10