Stats

  • Locked Locked
  • Replies 3
  • Subscribers 125
  • Views 16267
  • 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

Entering infoname and info (captab) analysis in ADE

RFStuff

Dear All,

I want to enter   infoname and info (captab) analysis in ADE (IC5141). 

I read through the Virtuoso Spectre Circuit Simulator User Guide there it gives an example of captab analysis as beow

 

 tran1 tran stop=1μ infotimes=[0.1μ 0.5μ] infoname=capInfo

capInfo info what=captab where=file file='capNodes'detail=nodetonode

 

I actually want to give the file name where it can save the cpatab outputs and also I want to print the capacitances of the specified nodes. For example cpacitance between I30/I5/I0/net-x &  I30/I5/I0/net-y.

I ADE transient analysis cpatab option, I couldn't find any place where I can give the file name and the node names.

Could anybody please tell how it can be done.

Kind Regards,

  • Andrew Beckett

    The way to do this is to create a file called "capInfo.scs" with this content:

     capInfo info what=captab where=file file="capNodes" detail=nodetonode

    (use double quotes rather than single quotes that you had in your example). 

    Then include this in your simulation by using Setup->Model Libraries to reference the file.

    Then on the transient analysis options form, go to the Additional Parameters field and enter:

     infotimes=[0.1u 0.5u] infoname=capInfo

    You can't fill in the infotimes field on the form, because that will automatically add an info analysis to output the DC op point info at that time, and set infoname for you - which isn't what you want. The captab support in the transient analysis doesn't support this because it assumes you'll be writing the output as a binary (PSF) format file so that the ADE post-processing can read it - and so doesn't offer the choice of writing to an ASCII file.

    Regards,

    Andrew.

  • RFStuff

     Dear Andrew,

    Thanks a lot for your reply.

    With setting  detail=nodetonode, it is writing ( looks like) all nodes ( a lot of nodes).

    Is it possible to write only a few nodes like :-  I30/I5/I0/net1 : I30/I5/I0/net2, I30/I5/I0/net6 &  I30/I5/I0/net7, etc..

     

  • Andrew Beckett

    I think you will always get the complete set of nodes - I don't think you can reduce it.

    Andrew.

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.