Stats

  • Locked Locked
  • Replies 2
  • Subscribers 125
  • Views 22419
  • 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 PSPICE or TI models into Cadence Virtuoso

Raffaele Aaron

Hi everyone,

I've started a few months ago working on Cadence Virtuoso 6.1.7 and I've been able to import models using this guide (e.g. this model), unfortunately it doesn't work for some particular .lib files.

In particular I'm trying to import this model file for the THS4521, but, although it's a pspice model, it won't simulate through ADE.

A subset of the errors output by the simulator are as follows:

Fullscreen error.txt Download 
Subset of errors found while running ADE


Error found by spectre in `FDA_HT3', during circuit read-in.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 343: The instance `XI85' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 344: The instance `XI56' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 349: The instance `XI16' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 352: The instance `XI11' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 354: The instance `XI60' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
Error found by spectre in `CMFB', during circuit read-in.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 109: The instance `XI1' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 120: The instance `XI5' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
Error found by spectre in `FDA_HT3', during circuit read-in.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 362: The instance `XI24' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 363: The instance `XI25' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 368: The instance `XI40' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
Error found by spectre in `OUTPUTCIR', during circuit read-in.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 179: The instance `XI25' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 180: The instance `XI23' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 199: The instance `XIVOL' is referencing an undefined model or subcircuit, `0.085'. Either include the file containing the definition of `0.085', or define `0.085' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 202: The instance `XIVOH' is referencing an undefined model or subcircuit, `0.085'. Either include the file containing the definition of `0.085', or define `0.085' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 215: The instance `XISOURCEVLIMIT' is referencing an undefined model or subcircuit, `35e-3'. Either include the file containing the definition of `35e-3', or define `35e-3' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 218: The instance `XISINKVLIMIT' is referencing an undefined model or subcircuit, `-35e-3'. Either include the file containing the definition of `-35e-3', or define `-35e-3' before running the simulation.
    ERROR (SFE-23): "LIB_FOLDER/THS4521/THS4521.LIB" 233: The instance `XI1' is referencing an undefined model or subcircuit, `PARAMS:'. Either include the file containing the definition of `PARAMS:', or define `PARAMS:' before running the simulation.




ALSO this type of errors:
Warning from spectre in `HPA_AND2':`I194.XI0.XI32.XAHDLI44', in `CMFB':`I194.XI0.XI32', in `FDA_HT3':`I194.XI0', in `THS4521':`I194', during hierarchy flattening.
    WARNING (SFE-29): "LIB_FOLDER/THS4521/THS4521.LIB" 471: Cannot set parameter `v'.
Error found by spectre in `HPA_AND2':`I194.XI0.XI32.XAHDLI44', in `CMFB':`I194.XI0.XI32', in `FDA_HT3':`I194.XI0', in `THS4521':`I194', during hierarchy flattening.
    ERROR (SFE-1997): "LIB_FOLDER/THS4521/THS4521.LIB" 471: I194.XI0.XI32.XAHDLI44.E1: parameter `coeffs': Behavioral expressions can not be assigned to netlist subckt or model parameters, only device instance parameters can use behavioral expressions.

Does anyone have any idea on how to import this model?

Thank you very much in advance,

Raffaele Aaron

  • You should reference the model either via the "PSpice Files" section of the Setup->Simulation Files in ADE or by creating a pspice view and pasting the model in that way (setting the view type as "Pspice" when creating the new view, and then switching into that view using either the view list or a config). Don't just include it as normal SPICE (because it's not - there's an explicit approach for including pspice models in spectre because they have additional syntax beyond Berkeley SPICE).

    Regards,

    Andrew.

  • in reply to Andrew Beckett

    Thank you very much Andrew, it worked!Thumbsup

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.