How to simulate the noise in time domain

EDAboard.com Forum Index -> RF, Microwave, Antennas and Optics -> How to simulate the noise in time domain

Author

Message

neo

Joined: 19 Aug 2004
Posts: 57
Location: Beijing

07 Feb 2007 7:00 transient noise simulation sigma-delta

i noticed some designers say they simulate the receiver noise, e.g. 400uV, how do they get that num, i mean, with LNA, Mixer, PLL, and even the ADC? i guess they use the transcient to simulate that noise, but how to get the noise in transcient?

zeol

Joined: 20 Jan 2006
Posts: 12
Helped: 5

07 Feb 2007 11:53 Re: How to simulate the noise in time domain

My guess is that they run the transient simulation and FFT the transient results, the noise floor from the FFT should be what they are referring to.

neo

Joined: 19 Aug 2004
Posts: 57
Location: Beijing

07 Feb 2007 16:34 Re: How to simulate the noise in time domain

but the transcient cannot simulate the noise,right? they only get the distortion, not the noise response!
but thanks all the same

khouly

Joined: 20 Oct 2003
Posts: 2479
Helped: 343
Location: EGYPT

07 Feb 2007 17:08 Re: How to simulate the noise in time domain

i think in agilent @DS there is transient noise simulation , but i didn't use it before , and don't know anything about the accuracy

khouly

Mazz

Joined: 03 Nov 2001
Posts: 592
Helped: 80

07 Feb 2007 17:55 How to simulate the noise in time domain

I think that a simulation with the complete receiver is almost impossible, if one ask for a reasonable accuracy.
Transient is for sure impossible.
The most probable solution is that the output noise (integrated over a certain bandwidth) is calculated from simulations of single sub-circuits noise figures and input noise.

This is a common approach, well consolidated.

I hope it can help.
Mazz

wpchan05

Joined: 16 Feb 2006
Posts: 165
Helped: 11

07 Feb 2007 19:37 Re: How to simulate the noise in time domain

SpectreRF can do noise calculation, and it can generate noise spectrum (provided you have the right noise parameters in your model file). The resulting noise floor is then found by integrating the noise spectrum over the freq region of your interest. Does it make sense?

neo

Joined: 19 Aug 2004
Posts: 57
Location: Beijing

08 Feb 2007 3:51 Re: How to simulate the noise in time domain

i think two tone transcient simulation of the complete receiver is acceptable, donnot think about the harmonic balance simulation to simulate a system more than two blocks.

some one really did simulate the noise performance by transcient, for example: Dennis Gee-Wai Yee of UCB in his PhD thesis (spring 2001) said he simulate the complete receiver noise figure of 5.7dB with sigma delta ADC, which i donnot know how, you guys know that? in my opinion, the transcient can only get the distortion information of the receiver and the quantization noise in the ADC

Added after 11 minutes:

Mazz wrote:

yes, we can cascade the performance, but it is not easy to mimic the real load between blocks, right? maybe you can give me an easy solution thanks Very Happy

Mazz

Joined: 03 Nov 2001
Posts: 592
Helped: 80

08 Feb 2007 9:59 Re: How to simulate the noise in time domain

On cascading blocks in RFICs, the most 'error free' approach is the simulation of output noise (or input referred, or Req) of each block, in addiction with each block gain (that can be also conversion gain).
Then use a simple formula to refer each block gain to the RF input (where you usually are matched) and convert it into noise figure, if you need it.
Then you can calculate accurately the overall noise of your system and so also the output noise.

Transient simulations, only with one tone are impossible. Suppose you have an RF (2.5GHz) tone, a PLL at 2.499GHz, an IF at 1MHz and the ADC. You need a time step very small to accurately simulate the 2.5 GHz signal and a stop time very large to get a significative number of 1MHz signal periods. 3 year simulation with a big server. No one does it.
Transient with noise sim are implemented in eldoRF, but their computational resources are very large, much larger than a simple transient.

I hope it can help.
Max

Sorry, but you need login in to view this attachment

neo

Joined: 19 Aug 2004
Posts: 57
Location: Beijing

08 Feb 2007 17:43 Re: How to simulate the noise in time domain

Mazz wrote:

u r perfectly right about the cascading noise using the noise voltage, i'd prefer the input refered noise instead of output noise because of the input noise's independancy of input source resistance, am i right, Mazz?

Mazz wrote:

Transient simulations, only with one tone are impossible. Suppose you have an RF (2.5GHz) tone, a PLL at 2.499GHz, an IF at 1MHz and the ADC. You need a time step very small to accurately simulate the 2.5 GHz signal and a stop time very large to get a significative number of 1MHz signal periods. 3 year simulation with a big server. No one does it.
Transient with noise sim are implemented in eldoRF, but their computational resources are very large, much larger than a simple transient.

I hope it can help.
Max

i did a transcient simulation to a receiver cascading of LNA+Mixer+VGA+Filter for a 10uS(just for functional verification), it took me 4 days long, i run this on a linux with 2.8G cpu and 2G ram, it seems acceptable

BTW, who has the slides which Chris Rudell in ISSCC2006 that discussed wireless standards and their impact on architectural choices? thanks

Last edited by neo on 09 Feb 2007 3:40; edited 1 time in total

estradasphere

Joined: 17 May 2005
Posts: 81
Helped: 2

08 Feb 2007 22:04 Re: How to simulate the noise in time domain

neo wrote:

Mazz wrote:

i did a simulation to a receiver cascading of LNA+Mixer+VGA+Filter for a 10uS, it took me 4 days long, i run this on a linux with 2.8G cpu and 2G ram, it seems acceptable

BTW, who has the slides which Chris Rudell in ISSCC2006 that discussed wireless standards and their impact on architectural choices? thanks

i think, mazz is right. it woudn't make sense to simulate the noise voltage with transient analysis? you can simulate the input or output referred noise voltage with "noise" or "pss/pnoise" analysis option in spectre. of course it would take too long (or is maybe impossible) to simulate LNA+mixer+vga+filter with pss, but you can simulate the noise voltages of LNA+mixer with "pss/pnoise" and the vga+filter with "noise" option in spectre. then you can numerically calculate the noise of the whole receiver chain. it would take maybe 2 hours instead of 4 days.

neo

Joined: 19 Aug 2004
Posts: 57
Location: Beijing

09 Feb 2007 3:42 How to simulate the noise in time domain

i am sorry for the misunderstanding, estradasphere
, i simulate the transcient, not the pss, it will be horrible to apply pss to the whole receiver

Google
AdSense
Google Adsense

09 Feb 2007 3:42 Ads

Mazz

Joined: 03 Nov 2001
Posts: 592
Helped: 80

09 Feb 2007 19:39 How to simulate the noise in time domain

neo
input referred noise is just output noise divided by small signal gain, so it should not depend on impedance. My suggestion is to use always source and load impedance in your sub-block noise simulations in order to take into account of real circuit conditions.

Another issue is simulation time: 4 days sims cannot be used to design, only for verification. By the way, why not a pss with LO tone only and a pac+pnoise to sim the overall receiver. I think that you'll get it in less than 4 days.

I hope it can help.
Mazz.