Stats

  • Locked Locked
  • Replies 2
  • Subscribers 125
  • Views 3149
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Transient Noise Simulation for Different input/output frequencies

EngrZM

hi

I am using virtuoso version IC6.1.5.500.16.2. I made a demodulator (60GHz Carrier , 20Gbps data rate) and trying to compare its output eye diagram with/without noise. 

I am using transient noise simulation and enabled the noise from frequency 40G (fmin) to 80G (fmax) with seed of 128 (seed is 128 because modulator has a PRBS source with 128 seed value).

By these values i am enabling the (white noise from 0 to 40G) + (white and pink noise from 40G to 80G) for the demodulator input signal.

But demodulator output signal  is 20G base band. How can i activate the noise (pink noise) for the output circuit elements which are dealing with 20GHz base band signal?

If i choose Fmin = 1Hz and fmax = 80GHz it enable white + pink noise from 1 to 80GHz but adds out band noise at the input of demodulator which is not desirable.

kindly give your valuable suggestion.

thanking you in anticipation

zubair

note: for transient noise simulation setup i studied the cadence document ""Application Note on Direct Time Domain Noise Analysis using Virtuoso Spectre"

  • Zubair,

    There are several things that I don't think you understand here - let me give some general pointers and then maybe you'll better know what to do:

    1. The seed for the transient noise analysis has absolutely nothing to do with the seed for the PRBS source. The PRBS source uses taps to feedback to generate a sequence of 1s and 0s, whereas the noise sources are generated using a floating point random number generator. There is rarely a need to set the seed, because the default seed ensures consistency of results; the only case it's really useful is if you are running multiple (shorter) simulations in parallel and want to get a number of results to average together rather than running one single longer simulation (this is how the choice for number of simulations works). So in your case, leave it alone.
    2. Setting noisefmin as low as 1Hz is of little value unless you simulate for the order of 1s - you wouldn't observe the effect of coloured noise at that low frequency unless you include at least one period of that frequency. Running a 1s simulator with time steps of around 6ps (2 per period of noisefmax) is going to be rather slow - that would be 160 billion time steps at least.
    3. That said, we now (in recent versions - IC617 together with SPECTRE161) set noisefmin to 1Hz by default rather than asking the user to enter it. This caused confusion and only saved a little simulation time with the improvements made in the analysis over recent years. So the noise you observe is going to be based on the duration of the simulation. 
    4. The noise you are generating comes from the devices - so trying to limit that to be within 40G to 80G is rather meaningless - you're not altering the noise at the source of the circuit, but the noise generated by the devices in the circuit. Even if you are only specifying noisefmin at 40GHz, it simply assumes the noise is white at frequencies below noisefmin (the documentation describes the noise power density as being constant below noisefmin). It simply uses the noise power at noisefmin at all frequencies below.
    5. So I'm not sure how meaningful it is to try to specify the noisefmin at some higher frequency because all it means is that your devices are potentially generating the wrong noise power at lower frequencies...

    Regards,

    Andrew.

  • in reply to Andrew Beckett

    dear andrew

    Many thanks for your kind guidance. I found the detailed and updated (2017) transient noise analysis document from cadence that has lot of valuable information which you beautifully summarized above. i will bother you for any further confusion. many thanks

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.