Stats

  • Locked Locked
  • Replies 5
  • Subscribers 125
  • Views 12435
  • 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

Importing and simulating .cir spice file in Cadence

delgsy

I am following the steps explained here.
But it seems that cadence cannot understand the resistor netlist expression.
I used the .cir file from here.

in .cir file:
Rxxx   terminal1   terminal2    r_model_name    r_value

in spectre:
Rxxx (terminal1 terminal2) resistor r=r_value

from log file:


I tried other way that is importing spice file from CIW.
It gives more problem, i.e., more errors, than the way I did above.

Is there anything that I can try?

Parents
  • ShawnLogan

    Dear delgsy,

    As noted in the link you included in your Forum post, did you add the following lines:

    simulator lang=spice
    **
    spice macro subckt netlist

    as the first few lines of the ".cir" file you referenced?

    Shawn

  • Andrew Beckett
    in reply to ShawnLogan

    Shawn,

    That shouldn't be necessary. Anything without a .scs suffix will be treated as SPICE anyway. I'm just doing some checks on the file to see how it behaves.

    Andrew

Reply
  • Andrew Beckett
    in reply to ShawnLogan

    Shawn,

    That shouldn't be necessary. Anything without a .scs suffix will be treated as SPICE anyway. I'm just doing some checks on the file to see how it behaves.

    Andrew

Children
  • ShawnLogan
    in reply to Andrew Beckett

    Dear Andrew,

    Andrew Beckett said:
    That shouldn't be necessary. Anything without a .scs suffix will be treated as SPICE anyway.

    I do recall you mentioning that to me sometime ago - but was not sure of the version of software delgsy was using and thought it worth at least trying. Thank you for your correction.

    Shawn

  • Andrew Beckett
    in reply to ShawnLogan

    Shawn,

    This has been the behaviour of Spectre for a good 20 years if my memory is correct (the .scs suffix only being used for spectre), so it's not due to the version number used.

    The issue is that you should treat the file as a PSPICE model (there's a comment in the model that also suggests that it's been tested with PSPICE). I tried running a quick command-line simulation using pspice_include in spectre and all ways OK.

    In the article pointed at, then for the various methods (each bullet number is the method in that article)

    1. Use -lang pspice with cdsTextTo5x
    2. Specify the type of the view as "Pspice" if creating a view this way
    3. In the last step, instead of including the file as a model library, use Setup->Simulation Files and include it in the pspice files
    4. Don't use this approach
    5. Or this approach - there's no PSPICE File->Import support

    Regards,

    Andrew

  • delgsy
    in reply to Andrew Beckett

    Hi Andrew, Shawn,

    I use method 3, put the .cir file in the Setup -> Simulation Files -> Psipice files, and without doing any modification on the original .cir file.
    It works.

    Previously, I used method 3 as well but put the .cir file as a model library.

    Thank you!

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.