Define subcircuit in Virtuoso Schematic using SPICE

Hi,
I'm using Affirma Virtuoso Schematic Editor to design the circuit
and later simulate using Spectre.
The question is that I want to put a subcircuit( an OpAmp), which is
defined in SPICE description from manufacturer. What instance should I
use in schematic and where should I put the text description? Is there
any other concern when using Spectre?
I really appreciate your help.

Lawrence

 

Andrew Beckett once wrote on comp.cad.cadence:
<quote>
1. Create a symbol for the component.
2. Copy that symbol to a view called "spectre" in the library manager
3. Do Tools->CDF->Edit CDF in the CIW
4. Change the form to "Base", and pick the cell.
5. Go down to the "Simulation Information" section, and click on the
Edit button.
6. Change the simulator to "spectre", and then:
Fill in the Terminal Order as the names of the symbol pins, in the
order in which they occur in the spice macromodel subckt header.
Either specify the component name as the name of the subckt, or
specify the component name as "subcircuit", and add a parameter
(further up the CDF form) called either "model" or "macro", where
the default value is the name of the subckt.

Then when you create a schematic, and have it wired up, and start
Tools->Analog Design Environment, you can then include the macro
model as a model file.
</quote>

The steps 3 to 6 can also be done by a SKILL file. The template is the
result of the cdfDump() command. (see cdfuser.pdf in documentation).
Create a textfile on disk and copy-paste the code to it. I have put some
comments into the code on the places where changes should be done. Don't
forget to create the symbol first. Then you load this modified code into
composer by load("filename").

The spice code (from .subckt to .ends) itself you put into another text
file and include it from the ADE->Setup->Model Libraries dialogue. You
may need to put a
simulator lang=spice
at the top of the spice file to avoid some warning messages.

--- 8< ---
/****************************************************/
;; Change library to a real library in your work environment
LIBRARY = "library_name"
;; Change CELL to be the name of the cell view that will be
;; black-box'ed
CELL = "cell_name"
/****************************************************/

let( ( libId cellId cdfId )
unless( cellId = ddGetObj( LIBRARY CELL )
error( "Could not get cell %s." CELL )
)
when( cdfId = cdfGetBaseCellCDF( cellId )
cdfDeleteCDF( cdfId )
)
cdfId = cdfCreateBaseCellCDF( cellId )

;;; Simulator Information
cdfId->simInfo = list( nil )
cdfId->simInfo->spectre = '( nil
;; Change termOrder to be the pin sequence defined
;; by the .subckt command.
termOrder ("PIN1" "PIN2" "PIN3")
;; Change componentName to be the name of the
;; subcircuit defined by the .subckt command
componentName "subcircuit"
netlistProcedure nil
)

;;; Properties
cdfId->formInitProc = ""
cdfId->doneProc = ""
cdfId->buttonFieldWidth = 340
cdfId->fieldHeight = 35
cdfId->fieldWidth = 350
cdfId->promptWidth = 175
cdfId->modelLabelSet = ""
cdfId->opPointLabelSet = ""
cdfId->paramLabelSet = ""
cdfSaveCDF( cdfId )
)
--- >8 ---