Stats

  • Locked Locked
  • Replies 7
  • Subscribers 126
  • Views 21314
  • 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

resistor noise simulation by transient analysis

rfham

Hi,

I am trying to run the simple example as depicted in the attached image, taken from Cadence's "Virtuoso Spectre Transient Noise Analysis" document, page 24.
link is support.cadence.com/.../ArticleAttachmentPortal;pageName=ArticleContent&sq=005d0000005nSd1AAE_20173303123103

But, I am not able to implement the resistor (with the user defined parameter kf) as required here!
here is my setup and simulation process:
1>insert instance "res" from analogLib in schematic editor

2>change its "model name" to say "res_mod" and also made a model file (res.scs)


3>then added this model file from ADE->Setup->Model Path. The text put in this model file is:


simulator lang = spectre
model res_mod resistor rsh=1k kf=10e-13

4>set following parameters at "tran" analysis.

I am getting error of following

looks the circuit is not stable, and i searched the forum and found the same topic of following link. but i cannot find the final solution.

https://community.cadence.com/cadence_technology_forums/f/38/p/31559/1340473#1340473

could you help to check this? thanks a lot.

  • Andrew Beckett

    I'm not sure what wasn't clear from my reply to the other post you mentioned. There appears to be a numerical instability with this trivially small circuit which shouldn't happen in real-life circuits which weren't just consisting of ideal components (ideal current sources). As I mentioned, changing the sine source to a voltage source also solves the problem - and for the purposes of illustrating how the transient noise works, that would be sufficient.

    If you see the problem with a real circuit, you should contact customer support.

    Of course, it would be good if we updated the support document to have a better example that didn't have this issue...

    Regards,

    Andrew

  • rfham
    it is very clear now, thanks a lot, Andrew.
    have a good day!
  • rfham
    hi, Andrew
    I have remove the isin source and replace idc by vdc and set the vdc =100mV, but cannot simulate the noise, for ideal current or voltage source, net current and voltage will be locked or clamp by the "ideal source", so if want to evaluate the single device noise level and characteristic, what's the most easy and right way to simulate noise in this case?
  • Andrew Beckett

    Plot the current through the voltage source, rather than the voltage across the resistor, which will of course be constant (because it's being driven by an ideal source). You can have the DC current source, plus a sine voltage source, but you'd still need to plot the current through the source or the current through the resistor.

    Regards,

    Andrew.

  • rfham

    hi, Andrew

    i got the new trans noise application note from cds website

    , and found the page 25 have the netlist as following:

    the netlist have two analysis, one is tran and another is tran noise,

    question one: how to set the two analysis above in one tran analysis GUI at ade explorer? i can set two test in ade assembler only like following figure

    question two: i cannot find the sweep_tran_noise-sweep, why not "tran"?

    how to add a_t_noisy- a_t expereesion, assembler can only add for test tran_noise or tran, cannot add this at high level.

     

     

    thanks a lot.

  • Andrew Beckett

    Answers:

    1. You can't do this in Explorer (at least not without using an include file to add the analyses). ADE limits you to a single analysis of each type (in general; there are a few exceptions for some of the RF analyses where special cases have been added to allow, say, multiple pnoise analyses).
    2. With the tran_noise test, if you turn on the "multiple run" option on the transient noise form, it will add a sweep of the iteration number around the tran analysis (look at the resulting netlist). However, you don't necessarily need to worry about the low level details - if you want to do a difference, simply add an expression to (say) tran_noise which is calcVal("a_t_noisy" "tran_noise")-calcVal("a_t" "tran"). calcVal allows you to reference results from other tests; you simply give the output name as the first argument and (optionally) the test name as the second argument. If you don't specify the test name, it refers to the same test the expression is used in. ADE will automatically ensure that the dependencies are met so that the analyses are run in the right order before calculations are performed.

    BTW, the forum guidelines ask you not to post on the end of old threads; this is a different topic so would have been better as a different thread. Still, it's done now...

    Regards,

    Andrew.

  • rfham

    Andrew, I’m truly grateful for your help, your reply teach me  lots of your knowledge.

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.