Home > Community > Forums > Custom IC Design > How to associate an extracted netlist of a subckt to the symbol view in schematic editor.

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 How to associate an extracted netlist of a subckt to the symbol view in schematic editor. 

Last post Sun, Mar 24 2013 4:09 AM by RFStuff. 8 replies.
Started by RFStuff 19 Mar 2013 06:29 AM. Topic has 8 replies and 1616 views
Page 1 of 1 (9 items)
Sort Posts:
  • Tue, Mar 19 2013 6:29 AM

    • RFStuff
    • Top 25 Contributor
    • Joined on Tue, Feb 5 2013
    • Posts 223
    • Points 3,930
    How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

    Dear All,

    I am using Calibre ( mentor Graphics). It creates the spectre Netlist and calibre view for PEX.

    However, claibre view creation takes a lot of time unlike its spectre Netlist.

    The spectre netlist it creates in a file like xyz.pex.netlist.

    The format is as below:-

     

    simulator lang=spectre
    include "SUBCKT_BLOCK.pex.netlist.pex"
    subckt SUBCKT_BLOCK (  DVDD DVSS A B C D E \
     F )

            .................................

    ............................................

    ............the sub ckt netlist body .............

    ........................................................

    include "SUBCKT_BLOCK.pex.netlist.DIV_BY_4_WITH_GRID.pxi"
    //
    ends SUBCKT_BLOCK
    //
    //

     

    Is it possible to associate this netlist to the corresponding subckt symbol used in the bigger ckt block the schematic editor so that the created netlist will have the above sub-ckt netlist in the output netlist of the bigger ckt block ?

    Kind Regards,

     

    • Post Points: 5
  • Wed, Mar 20 2013 7:39 AM

    • RFStuff
    • Top 25 Contributor
    • Joined on Tue, Feb 5 2013
    • Posts 223
    • Points 3,930
    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

    Dear All,

    I followed this link :- http://www.cadence.com/Community/blogs/rf/archive/2009/01/07/tip-of-the-week-how-to-simulate-a-subcircuit-netlist-with-spectre-in-ade.aspx,

    but it did not work.

    The model name is being written 'subcircuit'

    i.e in the netlist it shows something like I0 ( A B .......other terminals) subcircuit.\

    Subsequently in the ADE run I am seeing the error " that the model  subcircuit is NOt found".

    Could anybody please tell where I am going wrong.

    Kind Regards,

     

    • Post Points: 20
  • Wed, Mar 20 2013 8:07 AM

    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

    Hard to be 100% sure without seeing the CDF, but my guess is that you've left the component name as "subcircuit" in the spectre simulation information in the CDF, or have left the value of the "model" parameter blank. You could also just replace "subckt" in the spectre simInfo with whatever the subckt is actually called.

    Regards,

    Andrew.

    • Post Points: 20
  • Wed, Mar 20 2013 9:44 AM

    • RFStuff
    • Top 25 Contributor
    • Joined on Tue, Feb 5 2013
    • Posts 223
    • Points 3,930
    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

     Dear Andrew,

    Thanks a lot for your reply.

    May be I was unable to interprete the steps written in that page. So I am thinking better to post the steps I have alrady done.

    What I want :-

    a) I want to associate the extracted netlist file named  BLOCK.pex.netlist to the symbol BLOCK  ( which is being used in a bigger schematic) only when I want to do PEX simualtion of the entire big schematic.

    b) I should also revert back to normal symbol ( not PEXed netlist) view  when I am not interested in PEX simulation

    What I did is as follows:-

    1) I went to BLOCK_LIB-> BLOCK and copied the symbol of BLOCK  to spectre view. So a spectre view is created which is exactly like the symbol.

    By the way BLOCK_LIB is the library containing the cell  BLOCK. So what I did is:-

    BLOCK_LIB-BLOCK-Symbol   copied to  BLOCK_LIB-BLOCK-Spectre


       

    2) icfb->Tools->CDF->Edit ( CDF prompt came up)

    3) CDF Section->Cell                             CDF Type-> Base

    4) Browsed to the cell containing the symbol BLOCK.

    5) Then went to the Component Prameter Section

            clicked on Add button. Edit CDF Parameter Form came up

                param Type - string

               parseAsNumber- no

              parseAsCEL-yes

             storeDefault-no

             name-model

             prompt-BLOCK

              The remaining field I kept blank

              Clicked on  Apply

    6)    Then I went to Simulation Information Section

          Clicked on Edit button

          Edit Simulation Information Form came up

        Choose Simulator:- spectre

         otherParameters- model

        componentName- 

                             kept blank as suggested in that page, I think, Andrew you are pointing to this ( bang on target) which is by default subcircuit. Am I right ?

         termOrder- pins names filled in the proper order as in the .netlist file. i.e. "A"  "B" "C" "D"

        Rest kept blank

        Clicked on  Apply     

     

    Well That is it !!!

     

    issues:-

    1) The model name is coming as subcrcuit

    2) How I can revert back to the normal symbol view ?

    Kind Regards

     

        

            

             

    • Post Points: 5
  • Thu, Mar 21 2013 1:41 PM

    • RFStuff
    • Top 25 Contributor
    • Joined on Tue, Feb 5 2013
    • Posts 223
    • Points 3,930
    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

     Dear All,

     With changing the " componentName- to the Name of The CELL" ( as suggested by Andrew), it is taking the netlist file.

    But once the spectre view is created, the netlist always taking/ tries to take the model ( in my case the extracted big Netlist) even if you have both symbol view and spectre view of the cell. It doesn't distinguish between symbol view and spectre view as far as the netlist is concerned. If I disable the model ( the netlis), it still tries to take the netlist and gives error.

    Could anybody please tell how I can revert back to the normal symbol view operation without deleting the already created Spectre view ?

    Is there any simpler ways of inserting pin name into the cell view ? One can easily commit  a mistake while inserting pin name in order especially when the number of pins of the CELL is large ?

    Kind Regads,

    • Post Points: 20
  • Sun, Mar 24 2013 1:53 AM

    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

    I suspect you original problem was caused by adding a parameter "model" but not giving a value to the model parameter, and then it reverts to the default behaviour of using the componentName.

    Anyway, if you want to switch between the schematic and your "spectre" view, you can do one of two things:

    1. Use the hierarchy editor to create a config view for your design and then pick the "view to use" for the block in question. Then simulate in ADE from the configured design (open the config and make that the design in ADE).
    2. Use the switch view list in Setup->Environment in ADE and put "schematic" ahead of "spectre". 

    Regards,

    Andrew

    • Post Points: 20
  • Sun, Mar 24 2013 3:35 AM

    • RFStuff
    • Top 25 Contributor
    • Joined on Tue, Feb 5 2013
    • Posts 223
    • Points 3,930
    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

     Dear Andrew,

    Thanks a lot for your reply.

    When the number of pins are really large, entering the pins manually is painful and error prone.

    Is there a way other than manually, of entering the pins from the symbol.

    Kind Regards,

     

    • Post Points: 20
  • Sun, Mar 24 2013 4:01 AM

    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

    You could open the symbol, and do:

    artGenerateHierSymbolCDF(geGetEditCellView())

    and then you'd have to manipulate the order to match the external netlist.

    You could always write some SKILL to parse the subckt header and then do some pattern matching to the terminal names in the symbol and do this yourself...

    With QRC you can also specify the pin order that you want when doing the extraction; not sure if other extraction tools provide this (you'd have to ask the vendor) - that way you can generate the order in the CDF using the above SKILL function, and then give this order to your extraction tool.

    Kind Regards,

    Andrew.

    • Post Points: 5
  • Sun, Mar 24 2013 4:09 AM

    • RFStuff
    • Top 25 Contributor
    • Joined on Tue, Feb 5 2013
    • Posts 223
    • Points 3,930
    Re: How to associate an extracted netlist of a subckt to the symbol view in schematic editor. Reply

    Thanks a lot.

    Kind Regards,

    • Post Points: 5
Page 1 of 1 (9 items)
Sort Posts:
Started by RFStuff at 19 Mar 2013 06:29 AM. Topic has 8 replies.