How to determine capacitance of input pin with spectreS

Discussion in 'Cadence' started by Thomas Popp, Jul 21, 2003.

  1. Thomas Popp

    Thomas Popp Guest

    Hello,

    Can anyone give me a hint how I determine the capacitance of an input
    pin of a standard cell (extracted netlist) with spectreS?

    Thanks in advance for any help.

    Thomas
     
    Thomas Popp, Jul 21, 2003
    #1
    1. Advertisements

  2. Thomas Popp

    S. Badel Guest

    watch the net-list and add all capacitances connected to that node.
     
    S. Badel, Jul 23, 2003
    #2
    1. Advertisements

  3. Thomas Popp

    Thomas Popp Guest

    You mean I have to do it by hand??? Or is there a function in spectreS
    (OCEAN) which does the trick automatically? I've heard that a typical
    SPICE simulator is able to calculate the capacitance of every node of a
    given netlist. So I strongly presume this is also possible with spectreS...

    -Thomas
     
    Thomas Popp, Jul 23, 2003
    #3
  4. Thomas Popp

    S. Badel Guest

    don't know any special function. However, if you want to compute
    the parasitic capacitance at the input of a cell, you can do the following.

    open layout & schematic views
    run extraction on layout, then LVS
    LVS must be successful
    then, on LVS window select "parasitic probe", push "whole net" and select a
    net in
    the schematic. This will add up all parasistics and display the result.
    However, it non-parasitic capacitors won't be taken into account.
    hope this helps,
    s.badel
     
    S. Badel, Jul 24, 2003
    #4
  5. Thomas Popp

    Marc Heise Guest

    Thomas,

    I think you are looking for the "captab" function of spectre. Here is an
    example how to include it in a netlist for a DC run (it is not in the gui
    yet, so you might load it over an include file ):

    dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status \
    infoname=capinfo2
    capinfo2 info what=captab where=file file="capnodesdc"
    dcOpInfo info what=oppoint where=rawfile

    Regards,
    Marc



    Regards,
    Marc
     
    Marc Heise, Jul 24, 2003
    #5
  6. Thomas Popp

    Thomas Popp Guest

    Thanks a lot, that worked!

    But I had to do it slightly different: open layout - run extraction -
    open extracted view - open LVS window - select "parasitic probe" - push
    "whole net" and select a net in the extracted layout
    No schematic view or LVS-run was needed...


    -Thomas
     
    Thomas Popp, Jul 24, 2003
    #6
  7. The simples way is to run the simulation driving the input from a
    voltage source and integrate the current on the input pin.

    Two notes:
    - the precision of the simulation is very important;
    - the input cell capacitance may depend on the state of the other input
    pins (miller effect).

    Robert
     
    Robert Szczygiel, Jul 24, 2003
    #7
  8. Thomas Popp

    Thomas Popp Guest

    Thanks for your help Marc!

    Actually I'm running the simulation of my standard cells with OCEAN
    using the simulator spectreS.

    Until now I don't mess around with the simulation netlists. I get them
    by creating a simulation schematic for a cell and starting the "Analog
    Environment". Then I create a raw and a final netlist of the whole
    simulation circuit (using the extracted netlist of the simulated
    standard cell). These netlists are then used by a OCEAN skript to
    perform the simulation.

    My question is: Is it possible to use OCEAN to tell the simulator
    __spectreS__ to compute the capacitance of an input pin of the simulated
    standard cell?


    -Thomas
     
    Thomas Popp, Jul 24, 2003
    #8
  9. Thomas Popp

    Marc Heise Guest

    Hi Thomas,

    as far as I know captab did not exists in spectreS.
    The easiest would be what Robert suggestet. Let OCEAN do a simulation of a
    voltage source on your pin and do the postprocessing (integration) inside
    the same OCEAN script.


    Marc
     
    Marc Heise, Jul 25, 2003
    #9
    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.