Designer’s Guide Community

richard88

Community Member

Offline

Posts: 37

spectre noise sim for bandgap ref ?
Aug 21^st, 2006, 5:58pm

Hi,
I have a bandgap reference system that need to measure its noise output in uVrms using spectre. When I open the choosing Analyses option, what should I fill up the Output Noise & Input Noise portion ? For output noise, there is probe/voltage option and we need to select Output probe instance .... is it just selecting the output cap ?
For input noise, there is port/voltage/current and we need to select the corresponding input port, voltage source .... what should I select ?

Thanks !
Richard

Back to top

IP Logged

Ken Kundert

Global Moderator

Offline

Posts: 2386
Silicon Valley

Re: spectre noise sim for bandgap ref ?
Reply #1 - Aug 21^st, 2006, 9:40pm

For the output you can either select a pair of nodes or a probe component. If you select a pair of nodes the noise voltage across that pair will be calculated. If you select a probe in the form of a resistor, then the noise voltage across the resistor is calculated. If you select a voltage source or current probe as you probe, then the noise current through the probe is computed.

You only need to select the input if you are interested in computing the input referred noise, which you probably do not want for a bandgap. Any way, you would choose either a voltage source or a current source. You could also choose a port, in which case the noise figure is computed rather than the input referred noise.

-Ken

Back to top

IP Logged

richard88

Community Member

Offline

Posts: 37

Re: spectre noise sim for bandgap ref ?
Reply #2 - Aug 21^st, 2006, 10:44pm

Ken,
Thanks for the reply. Just wish to confirm, to see only the output referred noise, we can either the input noise port blank ? I think it would force me to enter something. If I choose a noise voltage source, say at VDD, I need to select an instance (vdc) ? I think my problem lies mainly on how to choose the input part.

Thanks,
Richard

Back to top

IP Logged

Ken Kundert Global Moderator Offline Posts: 2386 Silicon Valley	Re: spectre noise sim for bandgap ref ? Reply #3 - Aug 21^st, 2006, 10:47pm You should be able to not specify and input probe. -Ken
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: spectre noise sim for bandgap ref ?
Reply #4 - Aug 23^rd, 2006, 1:44pm

The form for noise analysis in spectre in the Analog Design Environment doesn't give a choice of "none" (yet). I filed a PCR recently (a few months ago) asking for precisely this.

In the RF analyses, there's a choice of none - and of course spectre itself doesn't need an iprobe to be set.

I just checked the PCR (887994) and it's been implemented in IC5141 USR4, due in the middle of September.

In the meantime pick some arbitrary source - it doesn't affect the output noise at all (which is the primary calculation). Do watch out if you're using a sub-version between IC5141 USR3 and 5.10.41.500.3.43 (when it was fixed) as there was a bug where the noise summary table couldn't be displayed if there was no gain between the input source and output - you got a divide by zero error.

Regards,

Andrew.

Back to top

IP Logged

richard88

Community Member

Offline

Posts: 37

Re: spectre noise sim for bandgap ref ?
Reply #5 - Aug 25^th, 2006, 6:12pm

Thanks for all the replies.
I'm able to run noise sims now Cheesy

, and I got the integrated output noise by Results->Direct Plot-> Output Equivalent Noise, later I clicked wave from calculator and print "sqr(integ(wavew10s1il()**2,10,100k)).

My problem now is :
I need to get the noise expression and put it in the "Setting Outputs" so that I can do Monte Carlo sim. However, as you can see, it would have a problem with the "wave" parameter. How can I put the noise expression into the calc then ?

Thanks,
Richard :)

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: spectre noise sim for bandgap ref ?
Reply #6 - Sep 5^th, 2006, 8:08am

Use Results->Direct Plot->Main Form, choose the noise analysis, and then turn on the "add to outputs" button. Then select the output noise you want to plot.

You'll get the expression for the output noise in the Outputs section of the ADE window - double click on the line in the outputs window and you can steal the expression. Use this instead of teh waveXXXX() function in your expression - you still need to do the integ() around this expression.

If I wasn't so lazy I'd check the expression and paste it here 8-)
Andrew.

Back to top

IP Logged