SPICE Library Import Procedure

To import a SPICE library or one of its components in a Circuit schematic:

1. View the Component Libraries. Open the Symbols area. Click Models.
2. From the area, select the Spice icon to open the Select Model File window.
3. The Files of type menu lists the file types for the SPICE file. You can import a SPICE library (.lib), a SPICE subcircuit definition (.cir, .spc, .sp), or a Spectre-format (.scs). You can specify the location of the SPICE file by clicking Use Path, PersonalLib, UserLib, or SysLib.
   Note:

   Import Spectre. Spectre-format files are case-sensitive.

Within the PersonalLib, userlib, or syslib folder, select the file from those listed, or type the name of the file in the File Name area. Note that syslib is reserved for libraries supplied with the Ansys Electronics Desktop (AEDT)^TM electronics systems design platform. See Paths for Model File Selection for details.

4. Click Open in the Select Model File window to open the Component Import window.

The Component Import window lists all the SPICE components that are contained in the library.

• Check a box in the Create Component column for each component you wish to import.
• Click the Symbol and Footprint column boxes to assign a symbol and footprint to a component. These steps are optional; if either one is left unspecified, a default symbol or footprint is created automatically.
• Select OK to import the selected components and thereby display their names in the Project Manager window.

Once the component has been placed in the schematic, its Property Window will show a checkbox property named NetlistAsSubcircuit. Enabling the checkbox affects only what is written to the netlist for simulation. When the checkbox is enabled, the Spice model component will be netlisted inside its own subcircuit along with its file reference. This means the model name (taken from the Spice file) cannot conflict with the same model name in a different Spice file netlisted for a different component. If two Spice files with identical model names are read into the global scope, only data from one of the spice files will be used for all components referencing that model name, causing a simulation error. Checking the ”NetlistAsSubcircuit” property will move the file out of the global scope and prevent this problem.

Grouped Components

From the Component Import window, select Group similar components in order to group components that have the same parameter names and values. Require consistent parameter values (enabled only when Group similar components is selected) enforces that every element in the group has the same parameter values, which is the default.

The criteria for grouped components are:

• Components must be selected for import.
• Components must have the same number of pins.
• Models must have the same base model type (cap, bjt, etc).

After selecting Group similar components in the Component Import window, similar components are grouped in the display:

• After grouping, the Name column displays the file name of the component group appended with a group number; you can change this name by typing in the Name column.
• Multiple groups can be found, but every element of a group must have the same grouping criteria.
• A group can only be created if it contains multiple components.

Select OK to import the component group and thereby display its name in the Project Manager window.

• After placing the component group in the schematic, the component possesses a special property, VComp, that is displayed in the Properties window. Click the VComp property to select which model in the group are used in the schematic.
• Click Choose Model in the Properties window to open a Model List window that displays all the models in the group.
• You can then select a new model, click OK, and the new model name are reflected in the Properties window.

5. If you do not select your own symbol for an imported component, a default symbol are automatically selected. To select your own symbol, click Symbol to open the Select Definition — Symbols window. For more information, see Using the Symbol Editor.
6. If you do not select your own footprint for an imported component, a default footprint are automatically selected. To select your own footprint, click Footprint. If you have encrypted libraries, this opens the Enter Password window.

After entering a valid password, or if you do not have encrypted libraries, the next window to open is the Select Definition — Footprints window. For more information, see Using the Footprint Editor.

7. If you select Check this box if this is a PSPICE component on the Component Import window, the component is imported as a PSPICE component.

The global tab of the netlist for the component includes lines (shown in bold) to switch to the PSPICE parser for this library, then back to Nexxim for the rest of the netlist:

simulator lang=pspice

.inc "C:\Documents\Ansoft\PersonalLib\Component Data Files\Component Data Files\Spice\BC8\\

57_PNP_Model.lib"

simulator lang=nexxim

For more information about AEDT libraries see Using the Component Editor.