Designer’s Guide Community

aidnaal New Member Offline Posts: 4	How to simulate thermal noise in SC circuits? Sep 12^th, 2007, 3:16am How can I simulate the thermal noise in SC circuits in HSpice?
Back to top	IP Logged

ywguo Community Fellow Offline Posts: 943 Shanghai, PRC	Re: How to simulate thermal noise in SC circuits? Reply #1 - Sep 12^th, 2007, 4:58am Hi, HSPICE has not the capability of simulating the thermal noise in SC circuits. You'd better try spectre. Yawei
Back to top	IP Logged

Frank Wiedmann

Community Fellow

Offline

Posts: 678
Munich, Germany

Re: How to simulate thermal noise in SC circuits?
Reply #2 - Sep 12^th, 2007, 6:24am

SpectreRF, to be more precise, see http://www.designers-guide.org/Analysis/sc-filters.pdf. For HSPICE, using transient noise might be a possibility. It's not my preferred way of doing such simulations due to the stochastic nature of the results and the fact that there is no listing of noise contributors available, but if only HSPICE is available, this might be the only way of getting a result at all.

Back to top

IP Logged

Monkeybad

Junior Member

Offline

Posts: 31

Re: How to simulate thermal noise in SC circuits?
Reply #3 - Sep 12^th, 2007, 8:25pm

Hi, aidnaal
You can try to use .NOISE ac analyze.
The more details you can refer to the HSPICE user manual.
It calculates the equivalent noise current multiply the output impedance.
Noise currents are due to thermal, shot or flicker noise.

In SC circuit, you can connect the circuit in unit feedback, so the printed result of the RMS noise voltage that HSPICE calculated means the total noise voltage reflected in the output node.

By the way, the flicker noise is proportional to 1/f, when you run .AC analyze, set your lower boundary frequency
in the proper value you interested. Or the HSPICE will calculate the unreasonable very large noise voltage because the flicker noise is very high in low frequency.
For example, when you design a ADC in 30MHz sample rate, then the lower boundary frequency can set to 30MHz, because in SC circuit the output voltage is changed every 30MHz due to sample and hold action. Only during hold action the SC circuit contributes the thermal noise.

It's just my way to do the noise analyze, correct me if I'm wrong. Thanks!

BEST REGARDS

Back to top

IP Logged

Frank Wiedmann

Community Fellow

Offline

Posts: 678
Munich, Germany

Re: How to simulate thermal noise in SC circuits?
Reply #4 - Sep 12^th, 2007, 11:24pm

A simple ac noise analysis will not give you the frequency translation effects that are typical for SC circuits. In principle, one could probably take the results of ac noise analyses for the different states of the circuit and then do the calculations described in section 2.2 of http://www.designers-guide.org/Analysis/sc-filters.pdf by hand, but I assume that this will be a lot of work and rather error prone.

Back to top

IP Logged