Transient Noise Analyses in Cadence

Normal transient analysis does not include any device noise (such as flicker, thermal and shot noise). To analyse noise, you either need to use a small-signal noise analysis (such as noise or for periodic circuits, pnoise/hbnoise or similar) - these are the most efficient ways of measuring the impact of noise on your circuit. For time-varying but non-periodic circuits, or for circuits where the circuit depends upon a large-signal response to the noise you can use transient noise - but this is generally the least efficient way of simulating the noise impact on your circuit. 

The reason why it's the least efficient is because to measure high frequency noise requires short time steps; to measure low frequency noise requires a large stop time. Both together will significantly affect the simulation throughput (no matter how efficient the transient noise implementation is in the simulator - which is pretty good in Spectre APS nowadays).

With modern versions you don't need to specify too much - you just need to specify the Transient Noise checkbox and fill in the Noise Fmax (the maximum frequency to generate noise at, which will influence the maximum timestep). You should be using an IC617 or later IC version, and SPECTRE16.1 or later.

Regards,

Andrew

Dear Mr. Andrew,

Thank you very much for your explanation.

Ok  now I understand that in normal transient simulation when I see any kind of distortion that is not at all related or contain noise information because the noise model of the devices is not modeled at the time of normal transient simulation, it is clear now for me. Then as you kindly said, to include the noise effect in my transient I must run the transient+noise analyses.

You kindly said "To analyse noise, you either need to use a small-signal noise analysis (such as noise or for periodic circuits, pnoise/hbnoise or similar), do you mean Sir by this simulation is the one by running the Noise analyses in ADE then I can find Input /Output referred noise, noise figure..etc. ??. 

Actually Sir my most concern is to measure the signal to noise ratio at the output of my amplifier, 

I have seen by Texas Instruments hand book that he divide the output signal range on the output referred noise (in this method I need to use the AC noise analyses I think !!).

Other people I see they use the FFT on the transient of the output signal, in this case then I must run transient with noise (the one you kindly suggested).

One more thing Sir, you kindly talked about step signal, people I see they use pure sin signal at the input when they run FFT

Thank you once again Sir

Signal to Noise measurements would also potentially include other unwanted noise such as quantisation noise in an ADC, which you wouldn't get by running noise analysis. So precisely what you need to do rather depends on what it is you're trying to measure. I would expect though for an amplifier you could compute it from the noise analysis results.

Andrew.

Dear Mr. Andrew,

For the Transient + Noise simulation,

You kindly suggested me to enter only the value of Fmax, and other boxes I leave it for default in my simulator. I am also using the Strobperiod in this way (1/8*F sampling or 1/16*F sampling) to be very much sure when I run the spectrum or DFT.

Please Sir if I want to perform the noise from 1 KHz to 10 MHz, in this case I will set the value of Fmax of the simulator to 10 MHz and the Fmin to 1 KHz. I read from the cadence documentation that inverse of Fmin should not exceed the transient stop time. is there any other parameters I should consider when I define Fmin ?

Which IC and SPECTRE versions are you using (please give the subversions - the IC version is in Help->About, and the Spectre version is at the top of the spectre.out file when you run from ADE)?

In current versions noisefmin defaults to 1Hz so you don't have to set it. In practice though you won't see the effect of low frequency noise unless you run a simulation for at least one period of that low frequency noise (even then you're not really going to see the effect with only a single period). So it doesn't really do any harm if the inverse of noisefmin exceeds the stop time - it just won't be observable.

Regards,

Andrew.

Dear Sir,

Thank you for your reply

OK, you're using old versions. I would advise using something more recent than 7 year old tools. If you really must use such old versions, you should set noisefmin because otherwise you won't see any flicker noise - it will just use the noise at noisefmax to set the noise spectrum as white across the entire frequency range. Decide what the lowest noise you need to see is, set noisefmin to that and then set the stop time to be 1/noisefmin.

Andrew.

Sir as you sked me before about what I need to measure and you kindly stated that if I am interested in to measure the SNR for an amplifier then the Noise Analyses will be possible, even more faster. but indeed I would also measure the THD, THD+noise of my amplifier and therefore I am using the Transient + Noise with the help of the spectrum I can different properties from one simulation  

Thank you Sir,

As I don't have an option to update the Cadence I will follow your procedure for the old one I use

Thank you a lot Sir