3 terminal nfet not netlisting correctly -> bn problem...

Discussion in 'Cadence' started by Spaceghost, Jul 11, 2004.

  1. Spaceghost

    Spaceghost Guest

    Hi all, I am trying to netlist a schematic with a 3 terminal mosfet. The
    problem is that the bulk node does not show up in the netlist and screws
    everything up. I looked at the CDF. There is a parameter called bn which
    is set by default to VSS. I'm doing a Spectre simulation and the bn value
    is passed in a statement that looks like D G S (progn bn). I looked around
    on the web and this is fairly standard. Cadence complains that the argument
    must be a string or number. I don't know what's going on but I think that
    somehow the body node is not getting passed correctly.

    This is really frustrating. The 4-terminal fet works just fine.

    Ideas?

    Thanks!
     
    Spaceghost, Jul 11, 2004
    #1
    1. Advertisements

  2. If I'm right here the programmable bulk node
    is not 'standard' for Spectre direct, but it is often used
    in SpectreS.

    For the Spectre netlisting process a lot of things has to be
    setup right.
    - symbol view
    - cell cdf (component description format) parameter and simInfo section
    - spectre stopping view

    And also this depends on the Design Framework version your are using.

    Form 5.0.32 up I thing there is the possibility to have the netSet
    datatype in your CDF.
    Then I suggest the following.

    Use a 3 term cell with a programmable bulk node
    - your symbol must have 3 terms D S G
    - your CDF must have a bn parameter
    in the component section
    paramType netSet
    name bn
    prompt Bulk node
    - your CDF must have the following entries in the
    simInfo for spectre
    termOrder D G S B
    termMapping nil D \:d G \:g S \:s B \:b
    - your spectre stopping view
    must have three terms D S G
    plus a fourth term B with a net expression
    Property name bn
    Default net vss/vdd -> depends on your mos type

    This should work.

    Bernd
     
    Bernd Fischer, Jul 12, 2004
    #2
    1. Advertisements

  3. Spaceghost

    Spaceghost Guest

    Bernd, thank you for the tips! I'm using Spectre instead of SpectreS, so
    that might be the problem! I am anxious to get back to the lab and check
    this out! :)

    Thank you for the help!

    Marc
     
    Spaceghost, Jul 12, 2004
    #3
  4. There is a 'Conversion Tool Box'
    under the Command Interpreter Windows 'Tools' menu.
    There you can find an item 'Analog Bulk Node Conversion ...'
    which might do the job for you or at least a part of the job.
    I can not give you more info on that because I never used it,
    I like to do such things manually, I'm not a friend of automated
    conversion because you can not look behind the scene.

    Bernd
     
    Bernd Fischer, Jul 12, 2004
    #4
  5. Spaceghost

    Spaceghost Guest

    I did some more checking today and I think there is an outdated cdsenv file
    which has to be deleted. Our sysadmin for some reason never works on Monday
    so I will have to wait.

    It turns out the simulator I am supposed to be using is Spectre.
     
    Spaceghost, Jul 12, 2004
    #5
  6. Spaceghost

    aznaragorn Guest

    I am having this same problem with the AMS netlister in Cadence
    because it doesn't suppport progn. I don't want to change hundreds of
    schematics to work with this inherited connects method. I changed bn
    to type netSet but what is the syntax for the netexpression i must set
    up in the Extra Terminals section of AMS Sim Info?
     
    aznaragorn, Jul 14, 2004
    #6
  7. Spaceghost

    Spaceghost Guest

    I'm using Spectre and when I made the net expression I just filled in a box
    with property name -> bn and default net VSS. I can check what the
    expression is when I head back to the lab!

    Marc
     
    Spaceghost, Jul 17, 2004
    #7
    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.