Stats

  • Locked Locked
  • Replies 2
  • Subscribers 63
  • Views 12320
  • 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

bbspice process failed

fastandig

I searched this and the RF forum, but couldn't find a discussion on this issue before. I am simulating a VCO test-bench with inductors extracted using EMX. I have the s-parameter file path entered as a variable for the n-port. When I start the simulation I get this error at the start almost immediately:

Error found by spectre during initial setup.

      ERROR (NPORT-1022): Generate lock-file for bbspice process failed.

Interestingly, when I simulate just the inductor n-port by itself with the same s-parameter file as above to get the Q and L, the simulation runs smoothly and I get the expected result. Another thing is that there are some older s-parameter files from last year that run perfectly fine with the above VCO test-bench. I'm not really sure what the problem is so would greatly appreciate some help. Thank you.

EDIT: If I change the n-port interpolation method to linear or spline the whole test bench simulation runs fine, but I would like to use bbspice for more accurate results.

  • Please download and review the AppNote: 7 Habits of Highly Successful S-Parameters (Spectre 20.1, 19.1 and IC6.1.8 ISR9) from https://support.cadence.com.   

    This goes into great detail about how to be successful simulating s-parameters in Spectre.  Typically we recommend you use the default interpolation method and let Spectre choose the interpolation method based on the analysis being run (there are exceptions to this - all discussed in the appNote).   Saying "would like to use bbspice for more accurate results" is not always an accurate statement.  :-)  

    Now about this error...

    I've seen this error happen when the user's disk quota is exceeded (the user deleted the contents under the ~/.cadence/mmsim/ directory to resolve the issue).   

    I've also seen the error when the permissions didn't allow data to be written to ~/.cadence/mmsim

    You can try the following.  Go to:  Simulation - Options - Analog, and on the Component tab set "nportirreuse" to "no".   And re-run the simulation.   Typically we *want* nportirreuse set to yes, as described in the appNote.

    best regards,
    Tawna

  • in reply to Tawna

    I found the problem. File path of a different user was specified under "nportirfiledir" because I had copied the test-bench. Once I removed the path, bbspice ran just fine.

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.