Stats

  • Locked Locked
  • Replies 9
  • Subscribers 126
  • Views 14815
  • 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

Spectre Simualtion errors (premature failure)

superman321
Im trying to simulate a simple Inverter with a spectre (version 5.1 ) and I have the following error messages: input.scs: (transistor nmos) T0 is an instance of an undefined model subcircuit. and similar error on the PMOS transitor too. Although, the same circuit was working fine a few days a ago. It has stopped suddenly with the above error messages. any help will be kindly appreciated. thanks

  • Check your model path and make sure you've set it correctly.  Also, you should be using MMSIM 7.1 spectre, not IC5141 spectre (which is quite old and out of date).

     

    best regards

    Tawna

  • Thanks, I have checked and rechecked my model file path, apparently, i works for my friend who is using the same model file, path and the spectre version 5.1..although I will check MMSIM 7.1 spectre!

  • Look in the netlist (input.scs) that's produced - is the path correct in the netlist? Does the file exist at that path? Do you have the right permissions to read it (although I'd expect an error if a specified file is not readable).

    Regards,

    Andrew.

  • Yes, I did look in the input.scs file..the file path is absolutely right and it has the right "read" permissions too...the circuit was simulating fine over the last two days and suddenly gave up on me today, although it still works fine for for friends who has the same "setup" file and the using the same model files as mine!
  • Andrew, my bad...i just figured that the input.scs does have the right model name and the netlister just names all the transistors as "subciruit" instead of "pmos" and the "nmos"...I made those changes in th input.scs file and its works fine. I have no idea why there are netlisting issues!..any clues?

  • Apologies - I thought I'd given the solution to this yesterday, but I accidentally appended the wrong post.

    So here's what I wrote:

    Sorry, I just realised I didn't read your original post closely enough. I spotted you said T0 is an instance of an undefined model subcircuit. The subcircuit is what gives it away - the netlist has ended up incorrect.

    Most likely this is because you don't have the UNIX environment variable $CDS_Netlisting_Mode set before you start virtuoso. Do:

    setenv CDS_Netlisting_Mode Analog

    (if using csh), or:

    export CDS_Netlisting_Mode=Analog

    if using bash/ksh.

    Then start virtuoso. 

    I suspect that will solve it. You'll need to do a Simulation->Netlist->Recreate to force it to renetlist.

    Regards,

    Andrew.

     

  • BINGO! BINGO!...it works like a charm..many thanks Andrew!
  • Andrew, here is an another question...can i set "setenv CDS_Netlisting_Mode Digital" , if so whats the difference btwn analog mode and digital?

  • You could, although that's exactly the same as it not being set. Digital mode means that netlisting is expected to be "NLP" rather than "CDF" based (it's for historical reasons).

    The practical consequence of this is that default values are not picked up from the CDF when in Digital mode; consequently if any instance's parameter values are at default, it doesn't look at the default value from the CDF, and just assumes it's not set. So what happens is that the "model" parameter (which is usually the default value, and not stored actually on the instance) gets omitted, and it falls back to printing "subcircuit" instead.

    So you don't want to be using Digital mode ;-)

    Regards,

    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.