Stats

  • Locked Locked
  • Replies 7
  • Subscribers 125
  • Views 26532
  • 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 terminated prematurely due to fatal error.

hTmTech
hello , 
I still have this simulation error message  " spectre terminated prematurely due to fatal error."  with cadence virtuoso
What is the problem ??
thanx 
  • Andrew Beckett

    The problem is that it terminated with a fatal error! Some error happened which was fatal...

    It would help to see the entire spectre.out log file to understand if it gives more information as to the reason.

    Andrew. 

  • hTmTech
    here the full error message :
     
     
    Cadence (R) Virtuoso (R) Spectre (R) Circuit Simulator
    Version 12.1.0.347.isr3 32bit -- 10 Jan 2013
    Copyright (C) 1989-2012 Cadence Design Systems, Inc. All rights reserved worldwide. Cadence, Virtuoso and Spectre are registered trademarks of Cadence Design Systems, Inc. All others are the property of their respective holders.

    Protected by U.S. Patents: 
            
     
     

    Includes RSA BSAFE(R) Cryptographic or Security Protocol Software from RSA Security, Inc.





    Simulating `input.scs' on ubuntu at 5:09:52 PM, Sun May 11, 2014 (process id: 2154).
    Current working directory: /home/htn/simulation/schema/spectre/schematic/netlist.
    Command line:
        /home/htn/htntools/mmsim/tools.lnx86/spectre/bin/32bit/spectre  \
            input.scs +escchars +log ../psf/spectre.out +inter=mpsc  \
            +mpssession=spectre0_1857_1 -format psfxl -raw ../psf  \
            +lqtimeout 900 -maxw 5 -maxn 5
    spectre pid = 2154

    Loading /home/htn/htntools/mmsim/tools.lnx86/cmi/lib/5.0/libinfineon_sh.so ...
    Loading /home/htn/htntools/mmsim/tools.lnx86/cmi/lib/5.0/libphilips_o_sh.so ...
    Loading /home/htn/htntools/mmsim/tools.lnx86/cmi/lib/5.0/libphilips_sh.so ...
    Loading /home/htn/htntools/mmsim/tools.lnx86/cmi/lib/5.0/libsparam_sh.so ...
    Loading /home/htn/htntools/mmsim/tools.lnx86/cmi/lib/5.0/libstmodels_sh.so ...
    Reading file:  /home/htn/htntools/simulation/schema/spectre/schematic/netlist/input.scs

    Time for NDB Parsing: CPU = 1.99612 s, elapsed = 8.79741 s.
    Time accumulated: CPU = 1.99612 s, elapsed = 8.79741 s.
    Peak resident memory used = 38.2 Mbytes.


    Error found by spectre during circuit read-in.
        ERROR (SFE-23): "input.scs" 12: PM0 is an instance of an undefined model pmos1.
        ERROR (SFE-23): "input.scs" 17: X0 is an instance of an undefined model f_opAmp.

    Reading link:  /home/ht/htntools//mmsim/tools.lnx86/spectre/etc/ahdl/discipline.h
    Reading file: /home/htn/htntools/mmsim/tools.lnx86/spectre/etc/ahdl/disciplines.vams
    Reading link:  /home/htn/htntools/mmsim/tools.lnx86/spectre/etc/ahdl/constants.h
    Reading file: /home/htn/htntools/mmsim/tools.lnx86/spectre/etc/ahdl/constants.vams

    Time for Elaboration: CPU = 36.002 ms, elapsed = 266.443 ms.
    Time accumulated: CPU = 2.03613 s, elapsed = 9.07521 s.
    Peak resident memory used = 40.7 Mbytes.

    spectre terminated prematurely due to fatal error.
  • Andrew Beckett

    hTmTech said:
    Error found by spectre during circuit read-in.
        ERROR (SFE-23): "input.scs" 12: PM0 is an instance of an undefined model pmos1.
        ERROR (SFE-23): "input.scs" 17: X0 is an instance of an undefined model f_opAmp.

     

    That explains it pretty clearly. This is why it's worth checking the whole file, not just the last line. You haven't specified your models. From the second one, I'm guessing you're using the (rather ancient) functional library. As described in the documentation for this library, you need to include:

    <ICinstDir>/tools/dfII/etc/cdslib/artist/functional/allFunc.scs

    in your model libraries (Setup->Model Libraries in ADE). Then it will find the definition of f_opAmp. Note however that this library contains very old macro-models which pre-date VerilogA (which is a far more powerful way of modelling behaviour).

    As for pmos1 - this is presumably related to the transistor you are using. I don't know whether this is from design kit or other, or a sample from Cadence - but you also need to locate and reference (via Setup->Model Libraries) the models that this uses. There is a model called "pmos1" in gpdk180 (the 0.18um Cadence Generic Process Design Kit), which you'd get if you included <GPDKinstDir>/models/spectre/gpdk.scs section NN in the model libraries. But I don't know if that is what you're doing. And if you're using gpdk devices, this should be added automatically when you start ADE.

    Regards,

    Andrew.

     

  • sona kaur
    in reply to Andrew Beckett

    hi sir i also have that same prematurely fatal error.. how to remove it??????

  • Andrew Beckett
    in reply to sona kaur
    sona kaur said:
    hi sir i also have that same prematurely fatal error.. how to remove it?

    Well, if it's the same "premature fatal error" as above, I explained above how to fix it. If it's not the same fatal error, you'll need to provide some details...

    Andrew

  • mohsinjutt
    in reply to Andrew Beckett

    hello sir i have the same error can you help me please

  • Andrew Beckett
    in reply to mohsinjutt

    Please read the rest of the thread in this post. If you have the same problem, then I explained how to fix it. If it's not the same error, then you'll have to provide the entire log file so that I can understand what the issue is and advise how to fix it.

    Oh, and the forum guidelines ask you not to post on the end (or in this case the middle) of existing threads.

    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.