Is there an easy way to simulate noise in spectre using measured noise

parameters?

--

S?ren Laursen http://www.tele.auc.dk/~slau/

Is there an easy way to simulate noise in spectre using measured noise

parameters?

--

S?ren Laursen http://www.tele.auc.dk/~slau/

Yes. Various sources in spectre (e.g. vsource, isource, port) accept a

parameter

noisefile which is a file containing spot noise data - see spectre -h

vsource

for more details, or look in openbook).

Of course, you need to be careful doing this. If the circuit you have

measured

noise data for has cyclostationary noise properties, and the circuit

you're analysing

in spectre is also periodic (with a related period to the measured

circuit), you

won't get the right answer, since you'll have lost important frequency

correlation

information when you captured the measured noise. The only real solution

in this case is to simulate the whole circuit.

If however, the measured circuit is not periodic, or the simulated circuit

is

not co-periodic with the measured circuit, then all should be OK. I'm

also primarily talking about the RF analyses here.

Regards,

Andrew.

> Is there an easy way to simulate noise in spectre using measured noise

> parameters?

> --

> S?ren Laursen http://www.tele.auc.dk/~slau/

> Yes. Various sources in spectre (e.g. vsource, isource, port) accept

> a parameter noisefile which is a file containing spot noise data -

> see spectre -h vsource for more details, or look in openbook).

> Of course, you need to be careful doing this. If the circuit you

> have measured noise data for has cyclostationary noise properties,

> and the circuit you're analysing in spectre is also periodic (with a

> related period to the measured circuit), you won't get the right

> answer, since you'll have lost important frequency correlation

> information when you captured the measured noise. The only real

> solution in this case is to simulate the whole circuit. If however,

> the measured circuit is not periodic, or the simulated circuit is

> not co-periodic with the measured circuit, then all should be

> OK. I'm also primarily talking about the RF analyses here.

> Regards,

> Andrew.

> > Is there an easy way to simulate noise in spectre using measured

> >noise parameters?

> > -- S?ren Laursen http://www.tele.auc.dk/~slau/

values of Fmin, Gammaopt, and Rn for a transistor at various

frequencies. If needed, these could be converted into a noise voltage

source, a noise current source, and a third noise current source. The

first and second noise source are correlated with a complex factor.

These three parameters are needed to fully describe a noisy two-port.

As a understand the documentation, the spot noise data file only

includes one parameter. Therefore, I can only simulate for a specific

load impedance.

Perhaps it is a limitation of Spectre? HPADS and other RF simulators

accepts noise parameters directly in a 2-port s-parameter file. Those

are not time-domain simulators, however.

--

S?ren Laursen http://www.tele.auc.dk/~slau/

Hi Soeren,

Currently this is a limitation of spectre's nport component - in current

releases

it is noiseless. In IC446 there will be some improvement (it can generate

thermal

noise itself, I believe), but not quite all the pieces are in place to

read the noise

parameters from the s-parameter file and use them - this is the subject of

several enhancement requests, and it should be coming in a future release

(I

believe it has been partially implemented, but is not completed yet).

That way it should be possible to describe the correlation between noise

as

well, and therefore not have loss of noise information in periodic

systems.

Regards,

Andrew.

> What I have as input is really measured s-parameters and corresponding

> values of Fmin, Gammaopt, and Rn for a transistor at various

> frequencies. If needed, these could be converted into a noise voltage

> source, a noise current source, and a third noise current source. The

> first and second noise source are correlated with a complex factor.

> These three parameters are needed to fully describe a noisy two-port.

> As a understand the documentation, the spot noise data file only

> includes one parameter. Therefore, I can only simulate for a specific

> load impedance.

> Perhaps it is a limitation of Spectre? HPADS and other RF simulators

> accepts noise parameters directly in a 2-port s-parameter file. Those

> are not time-domain simulators, however.

> --

> S?ren Laursen http://www.tele.auc.dk/~slau/

1. simulating phase noise in Spectre

Hi,

I am able to see flicker noise upconversion in my phase noise

simulations. However, the noise amplitude starts off from a value way

higher than 0dB (about 60-70 dB). The output is supposed to be in

dBc/Hz. So, should it not be less than 0dB at all times? I have tried

improving the tolerances but it is to no avail. Can someone suggest

something?

thanks

vivek

3. Does the phase noise simulation in cadence include 1/f noise upconversion?

4. Convert PackRat Addresses to Pilot?

5. Simulating Noise for VerilogA model

6. Legend of Blacksilver, Legacy of the Ancients, Crown Rebellion

7. phase noise in ring oscillator using spectre..

8. Thermal/shot noise simulation in Spectre

9. Problem using Spectre and SpectreS model to simulate

11. plotting phase noise through calculator

12. Plotting noise analysis results in Artist

4 post • Page:**1** of **1**