Stats

  • Locked Locked
  • Replies 4
  • Subscribers 125
  • Views 16530
  • 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

Post-processing non-PSF results formats through OCEAN

mnabil

Hi,

This seemed like a trivial question but I couldn't find an answer on the forum or online. In ADE you can simulate using spectre or HSPICE and you can still plot the results. I need to do the post-process the data through an OCEAN script. It is very easy to do so on results in PSF format by openResults("results_dir/psf") and then selectResult("analysis") of choice. Upon using HSPICE, the results are available in .tr0, .ac0 formats (even Spectre can output the results in these formats). I could not figure a way to process these formats and plot it on Virtuoso Waveform Graph XL.

Can you please let me know how to post-process these .tr0, .ac0 ...etc. formats using OCEAN? 

I'm using  HSPICE 2012.06-SP2 and IC6.1.5-64b.500.14 

 Thanks 

  • For more description of the issue, I keep getting this message: WARNING (OCN-6040): The specified directory does not exist, or the directory does not contain valid PSF results. Ensure that the path to the directory is correct and the directory has a logFile and PSF result files. I also tried ".OPTION PSF=2" to generate the outputs in ASCII format rather than binary, but that didn't help either. I'd appreciate anyone's help on this Thanks
  • Dear all,
    I found a way for converting a single .tr0 or .ac0 ..etc file into PSF format. It is through using HSPICE conversion function and I couldn't find a solution by cadence yet.
    Th function as listed in the HSPICE manual:
    converter -t PSF -i input_file <-o output_file>

    Example
    converter -t PSF -i testpost.tr0 -o testpsf

    The input file is testpost.tr0, which HSPICE generates with the POST option. The output file name is testpsf. After running, HSPICE generates two new files: testpsf.psf and logFile. The testpsf.psf file is a PSF file that you can view. The logFile is necessary for the AWD to load the waveform.

    However the input .tr0 file must be in ASCII format rather than binary format, so you have to use these to options:
    .OPTION ARTIST=2
    .OPTION PSF=2


    That worked well for a single .tr0 file. Howver I tried with a .tr0 that had a sweep variable built in and that didn't work properly. I I find an alternative way I'll post here.

    If you have an alternative way please share it here as well. I expect that there might be a conversion utility through Cadence itself.

    Thanks,

  • The .tr0, .ac0 files are Synopsys proprietary formats for HSPICE, and as such, ViVA does not read them. However, HSPICE can output PSF directly, and that would normally be done by setting:

    .OPTION ARTIST=2 PSF=2

    If it is not writing PSF, then you should contact Synopsys. As you say, the alternative is to use Synopsys' translator - Cadence do not provide a translator for the same reason; we provide libraries to allow third-party simulators to write a format that ADE/ViVA can read.

    Regards,

    Andrew.

  • Hi Andrew,

     It turned out that I don't need the conversion tool at all and that HSPICE can output the PSF format directory. I mistakenely had .OPTION POST =1  in my stimulus file which was changing the output format.

    Just setting .OPTION ARTIST=2 PSF=2 is suffiecient as we have both mentioned.

    Thanks,

    Mohamed 

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.