How to Simulate a Subcircuit (Netlist) With Spectre in ADE

Many users ask, "How do I instantiate a netlist into my schematic and simulate with spectre in ADE?"

To instantiate a subcircuit (netlist) in your schematic and simulate with spectre in ADE you need to create a cell with a CDF parameter 'model' which will point to the text subcircuit that you want to use for simulating. Here is the recipe:

1. Create a symbol view for the text subcircuit.
2. Make a copy of this symbol view and call the new view "spectre."
3. Open the base CDF for the cell, add a component parameter called "model."
4. In the Add CDF Parameter form, specify only these values in order:
   • paramType:string
   • parseAsNumber:no
   • parseAsCEL:yes
   • storeDefault:no
   • name:model
   • prompt:Model Name
5. Click "Apply"

This parameter holds the name of the subcircuit file to use during simulation for this cell.

Edit the simInfo section of the netlist for the spectre simulator (assuming you will simulate in spectre)

You must modify the simulation information to recognize the model property and support the parameters passed into the subcircuit file.

1. For example, in the Simulation Information section of the form, click Edit.
2. Update the following fields in this order (insert your own name for myParameters if you have instance parameters and insert your own terminal names for termOrder):
   • Choose Simulator: spectre
   • otherParameters: model
   • instParameters: myParameters
   • componentName: (leave blank)
   • termOrder: "input1" "input2" "output"
3. You also need to define your terminals (termOrder).
4. Instantiate the created symbol in a schematic and give the name of the subcircuit as the model name.
5. Then in ADE, provide the path to the file containing the text description of the subcircuit (i.e. the netlist) through Setup -> Model Libraries.

Note: if the netlist is in spice syntax, at the top of the file you should add the following statement:

simulator lang=spice

For more information, similar tips, and design topics, please visit Cadence Blogs and Technical Forums.

Related Resources:

• Spectre Circuit Simulator
• Virtuoso ADE Product Suite