Virtuoso AMS Environment User Guide

Using Existing Designs in the AMS Environment

Using Analog Primitives

Analog primitives must be converted for use in AMS Designer. To do the conversion, you use the Conversion Tool Box, which is opened by choosing Tools – Conversion Tool Box from the CIW and then clicking AMS simInfo from Spectre. The tool box operates on an entire library at a time so the library must contain only analog primitives. For more information about using the Conversion Tool Box, see “Converting an Existing Analog Primitive Library” on page 598

This tool box assumes that the primitives to be converted are already prepared for use with

Spectre Direct. If this is not true, you can

■Use another conversion tool to prepare the primitives for use with Spectre Direct and then do the conversion for AMS. For details about preparing primitives for use with Spectre Direct, see the “Preparing Files for Direct Simulation” section, in the “Converting Design Libraries and Technology Data” chapter of the Compatibility Guide.

■Manually create AMS simulation information for the primitives according to the definitions in Appendix B, “Updating Legacy SimInfo for Analog Primitives,” then use the steps in “PlacingSPICE and Spectre Netlists and Subcircuits in a Schematic” on page 189 to edit the CDF simulation information.

Using SPICE and Spectre Netlists and Subcircuits

This section describes briefly what you must do to use subcircuits, models, and netlists written in SPICE or Spectre. For additional information, see the “Using Subcircuits and Models Written in SPICE or Spectre” section, in the “Instantiating Analog Primitives and Subcircuits” chapter of the Virtuoso AMS Simulator User Guide.

Preparing to Use SPICE and Spectre Netlists and Subcircuits

To prepare to use a subcircuit or a model written in SPICE or Spectre, you must

1.Include the netlist or subcircuit in a model file.

The contents of the model file must be in Spectre or SPICE syntax. Spectre files should start with simulator lang=spectre and SPICE files should start withsimulator lang=spice and end with simulator lang=spectre. This practice protects against an inadvertent language change.

2.Give the elaborator the location of the model file.

Virtuoso AMS Environment User Guide

Using Existing Designs in the AMS Environment

You can meet this requirement either manually or by using the windows provided by the

AMS environment.

You can give the location manually by defining theMODELPATH variable in the hdl.var file, or by using the-modelpath option for ncelab. For example, an entry in the hdl.var file might look like this:

define MODELPATH model_filename

You can use the Analog Model Files form. For more information, see “Specifying Model Files to Use During Elaboration” on page 219.

Placing SPICE and Spectre Netlists and Subcircuits in a Schematic

After preparing as described in the previous section, you can add a SPICE or Spectre netlist or subcircuit to a schematic. To do so, you

1.Create a symbol for the netlist or subcircuit.

You can use the Library Manager to copy an existing symbol, then modify the new symbol as necessary.

2.Add the CDF termOrder field simulation information for the symbol.

a.From the CIW, choose Tools – CDF – Edit. The Edit Component CDF form opens.

b.In the Edit Component CDF form, select Base for the CDF Type.

c.Type in the names of the library and cell that hold the newly created symbol view.

d.Scroll down to the Simulation Information section and click Edit. The Edit Simulation Information form appears.

e.For the Choose Simulator field, selectams.

f.Type the terminal names into the termOrder field.

Neglecting this step causes compilation errors such as

In AMS, named port association for analog primitives is not supported.

3.If your SPICE or Spectre netlist or subcircuit supports models (as, for example, the bjt and resistor do),

Virtuoso AMS Environment User Guide

Using Existing Designs in the AMS Environment

a.Type model into the instParameters and otherParameters fields.

This tells the netlister that there is a model associated with the symbol.

b.Type a t into the isPrimitive field.

This tells the netlister to translate the cell to a Spectre primitive that supports models.

At the end of this series of steps, the Edit Simulation Information form might look like this.

Virtuoso AMS Environment User Guide

Using Existing Designs in the AMS Environment

4.If you are placing a Spectre built-in primitive that does not support models (such as vdc or vsin), type the name of the primitive into the componentName field.

5.Click OK to close the Edit Simulation Information form.

6.In the Edit Component CDF form, click Add to open the Add CDF Parameter form.

Type in any required parameters. When you close the form, the added parameters appear in the Component Parameters pane of the Edit Component CDF form.

7.Close the Edit Component CDF form, by clicking OK.

8.Place the symbol in your schematic.

For more information about this step, see the “Creating Schematics” chapter of the

Virtuoso Schematic Editor User Guide.

Virtuoso AMS Environment User Guide

Using Existing Designs in the AMS Environment