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

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,

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.

 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

 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,

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

 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,

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.

Thanks a lot.

Kind Regards,