Using Spice Macromodels in Cadence

Hi,

I have the spice macromodel of the device I want to simulate. What is
the way to use Spice macromodels in Cadence simulations (I don't want
to convert the code into schematic)?

Umut

 

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.

A little brief explanation (but it's from memory)...

Regards,

Andrew.