How to run simulation with spice netlist coming from dracula lpe drawing?

Discussion in 'Cadence' started by tech11, Dec 11, 2005.

  1. tech11

    tech11 Guest

    After run lpe drawing with dracula, I get one spice netlist which including
    parasitical cap and res. But when I run simulation with spectre and get
    errors such as 'spectre section definition not found' and many syntax
    errors. I remember spcetre can read spice netlist well, why does it output
    such errors? Need I deal with the drawing spice netlist? How should I do it?
    Since I have not done such one flow and would you please help me or give me
    some advice? Thanks for your help!

    Have a good day!

    Best Regards,

    Joffre
     
    tech11, Dec 11, 2005
    #1
    1. Advertisements

  2. Well, without seeing an example netlist, I don't know. You must be doing
    something to the netlist, since it wouldn't have analysis statements within it,
    nor would it have model references. It sounds as if you're trying to include a
    section of a model file, but are specifying it incorrectly.

    Note that files with the .scs suffix are interpreted as spectre syntax;
    everything else is SPICE. You might also want to use IC5141 and
    the +csfe command line option to spectre, or MMSIM60 where +csfe is on by
    default (this is the new front end which parses SPICE more completely).

    Regards,

    Andrew.
     
    Andrew Beckett, Dec 11, 2005
    #2
    1. Advertisements

  3. tech11

    tech11 Guest

    Well, without seeing an example netlist, I don't know. You must be doing
    Dear Andrew,

    Below is my spectre running spice netlist and run file:
    1) lpe extract file 'LPENET.sp':
    * CADENCE/LPE SPICE FILE : LPENET
    * DATE : 6-DEC-2005
    *
    ******
    ****** MOS XTOR PARAMETERS FROM : 7MOSXREF
    ******
    *
    *
    *.GLOBAL GND VDD
    *
    *
    ..SUBCKT .......
    ****** RESISTORS PARAMETERS FROM : 7RESXREF
    ******
    *
    *
    RI18 ZT<4> GND RH 1.40000E05K
    ........
    ****** BJT XTOR PARAMETERS FROM : 7BJTXREF
    ******
    *
    *
    QQ2 GND ZT<2> ZT<3> PN $EA=195.84P $EP=81.60U
    ........
    ****** CAPACITORS PARAMETERS FROM : 7CAPXREF
    ******
    ******
    ****** CAPACITORS PARAMETERS FROM : 7CAPXMER
    ******
    *
    *
    C1 XI0-XI2-NET265 GND 1.19480E-12PF
    .......
    *
    ..ENDS


    The spice netlist 'input.sp':
    // Generated for: spectre
    // Generated on: Dec 6 18:00:12 2005
    // Design library name: xxxxxx
    // Design cell name: xxxxxx
    // Design view name: schematic
    simulator lang=spectre
    global 0
    include $CDS_INST/tools.lnx86/dfII/samples/artist/ahdlLib/quantity.spectre"
    include "./LPENET.sp"

    parameters esr=20m iout=30m
    include "....model/.../xxx.scs" section=tt_bt_rt

    // Library name: xxxxxx
    // Cell name: xxxxxx
    // View name: schematic
    ......................

    The run file 'runs':
    spectre +spp +escchars +log ../psf/spectre.out
    +mpssession=spectre1_25233_40 -format psfbin -raw ../psf input.sp

    Then I run 'runs' directly
    $> ./runs
    //--INFORMATION--// SPICE Reader : MDL @version 1.2.2 01/31/2003

    //--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
    //--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
    //--FATAL ERROR--// SPICE Reader : Spectre section definition not found.
    //--WARNING--// SPICE Reader : ./LPENET.sp", Line 12 : zt<2> contained
    misused > operator!
    .........................................

    I don't know what's the reason and how to continue to finish the simulation.
    Would you please help me or give me some advice? Thanks for your help!

    BTW, do you know how to do the flow with hspice?

    Have a good day!
     
    tech11, Dec 12, 2005
    #3
  4. Unfortunately you've cut so much out of the netlist, that I can't really see
    what's wrong. I tried taking what you'd done and hacking it together. I get some
    warnings about the "misused > operator", but the main problem is the same as one
    I get when I try to run with the (better) spectre +csfe:

    spectre +csfe test.scs

    Error found by spectre during circuit read-in.
    "./LPENET.sp" 17: An exponential format number was found with an alphabetic
    suffix (1.40000E05K).
    "./LPENET.sp" 30: An exponential format number was found with an alphabetic
    suffix (1.19480E-12PF).


    I essentially get the same error with spectre +spp too:

    Error found by spectre in `blah', during circuit read-in.
    "./LPENET.sp" 17: An exponential format number was found with an alphabetic
    suffix (1.40000e05K).
    "./LPENET.sp" 30: An exponential format number was found with an alphabetic
    suffix (1.19480e-12p).

    It's not surprising - the values have an exponent _and_ a suffix. I don't think
    that makes sense... sounds as if something is wrong in your Dracula LPE setup.

    I don't get any errors due to sections - so there must be something else wrong
    in your netlist - or perhaps it's because you're using some older version with a
    bug (you don't say what version you're using).

    Can you try using +csfe like I suggested? (obviously you'll need to fix the
    values, otherwise you'll hit the problem I did).

    Andrew.
     
    Andrew Beckett, Dec 12, 2005
    #4
  5. tech11

    tech11 Guest

    Unfortunately you've cut so much out of the netlist, that I can't really

    Dear Andrew,

    Sorry for the cutting netlist! Since I'm not a designer and just try to help
    to test this flow, so it's inconvenient to post the full netlist and lpe
    result.

    Our tools is IC5033, I have no way to try the latest version. Would you
    please share your post-simulation steps with spectre? I have not do such one
    flow and don't know how to deal with the lpe results. Need I deal with the
    lpe-after spice netlist before reading in by spectre? May the spectre models
    be used by hspice?
    Is my run file right?

    When I run simulation with spectre? Does I need the schematic netlist?

    Sorry to trouble you so much!

    Have a good day!

    Best Regards,

    Joffre
     
    tech11, Dec 15, 2005
    #5
  6. tech11

    tech11 Guest

    Dear Fogh,

    Thanks for your reply! I lose to input the left quota, but there's it in my
    running file, so it's not the real reason. Have you go this flow and help
    me? Thanks a lot!

    Have a good day!

    Best Regards,

    Joffre
     
    tech11, Dec 16, 2005
    #6
  7. tech11

    fogh Guest

    Joffre ,

    I can t make tests for you. As Andrew pointed out, the main problem
    seems to be that numbers have both scientific notation and a suffix.
    This is to be adressed by LPE deck author. If he is not available, you
    ll have to get the LPE file, the dracula manual on the side, and start
    hacking ...
    If you are not up to delving in dracula, and find those numbers'
    format to be rather uniform, you can also try some regexp fix, stg like
    s/([ =][0-9][.][0-9]+E[+-]?[0-9]+)[aAfFpPnNuUmMkKgGtT][^ \t]*/\1/
     
    fogh, Dec 17, 2005
    #7
  8. Just doing a bit of catching up, and I just noticed that I didn't answer this -
    probably because I didn't understand the question...

    Andrew.
     
    Andrew Beckett, Jan 12, 2006
    #8
    1. Advertisements

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.