Couldn't access full transient simulation data

Discussion in 'Cadence' started by bageduke, Jul 5, 2008.

  1. bageduke

    bageduke Guest

    I am doing long transient simulation for 100us. The simulation is
    still running, but everytime when I tried to plot signal, it only
    plotted up to 36us, but actually output log shows the simulation
    already run more than 50us without any error, and the transient result
    file size still keep increasing.

    Have you ever seen this problem before? Does this mean the result is
    corrupted? Or is there anyway I can fix the problem?

    Thanks a lot.
     
    bageduke, Jul 5, 2008
    #1
  2. bageduke wrote, on 07/05/08 02:44:
    Are you using IC5141 with spectre from an MMSIM release? If so, you probably
    need to re-enable the "chunk" mode for writing PSF. In older spectre versions,
    big files used to get split into 2Gbyte chunks, because large file support was
    not particularly common in many OS versions. However, that's no longer true - so
    spectre from MMSIM61 changed to write large transient PSF into a single big
    file. However, support for reading such big files wasn't added into IC61 (I
    think), and so if running a new spectre with IC5141, you need to do:

    For Spectre writing PSF data:

    setenv PSF_WRITE_CHUNK_MODE_ON true

    For UltraSim writing PSF data:

    setenv PSF_LARGE_FILE_ON false

    Regards,

    Andrew.
     
    Andrew Beckett, Jul 7, 2008
    #2
  3. bageduke

    david.garner Guest

    Hi Andrew,

    I have a similar problem. I am simulating a sigma-delta converter and
    only the first 19 clock cycles would be displayed, despite simulating
    for 1024 or more, and the simulation clearly running through to
    completion.

    I enabled the above environment variables and found that I could see
    the first 177 cycles in AWD - a vast improvement - and the entire
    waveforms in Wavescan. But any calculator functions I do on those
    waveforms are only using the first 177 cycles.

    This does not appear to be related to the tran.tran file size - I have
    tried using various errprst settings and only saving every 10 points,
    etc.

    Any ideas?

    David.
     
    david.garner, Sep 3, 2008
    #3
  4. I've just found some issues related to changing the stop time when using SST2.
    The problem seems to be that the wrong precision gets used if you lengthen the
    stop time, and what can happen is that the x-values hit the 64 bit limit with
    the original precision (summarizing it slightly). This is covered in CCRs 574546
    and 517273 - for reference if you contact customer support.

    This has just been fixed in IC 6.1.2.500.17 - but I don't believe it is due to
    be fixed in IC5141 at the moment.

    Probably the simplest thing would be to change the output format to PSF. Use
    the following .cdsenv:

    spectre.envOpts simOutputFormat string "psfbin"

    or the following SKILL in your .cdsinit:

    envSetVal("spectre.envOpts" "simOutputFormat" 'string "psfbin")

    (note, you can't change this if you're already running ADE). You'll most likely
    need to force a new netlist (Simulation->Netlist->Recreate) to ensure the
    mappings are updated correctly.

    Best Regards,

    Andrew.
     
    Andrew Beckett, Sep 12, 2008
    #4
Ask a Question

Want to reply to this thread or ask your own question?

You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.