Exporting IFF Schematic Files from ADS for Mentor Graphics

This chapter describes the procedure for exporting an Intermediate File Format (IFF) schematic from Advanced Design System.

IFF Schematic Export from ADS

The basic procedure for exporting an IFF file from ADS can be broken down into several simple steps:

Exporting an IFF Schematic File

This section describes the procedure for exporting an IFF schematic file from Advanced Design System using the IFF Translator's User Interface. Before exporting an IFF schematic file, refer to Opening an ADS Project and Schematic Window.

Accessing the Schematic Export dialog

To access the schematic export dialog, launch your export from an ADS Schematic window.

Open your ADS Schematic Design in the ADS Schematic window.
Choose File > Export. The schematic Export dialog box appears.

Specifying the Export File Selection

In the schematic Export dialog box, choose the type of file to export, specify the new file name, and supply other basic information needed by the translator.

In the Export dialog box, select IFF from the File Type drop-down list if it isn't already displayed.
To specify the path and filename of the file you want to export, click Browse in the Export dialog box. The Export File Selection dialog box appears.
Double-click as needed to locate the directory for your exported IFF schematic file in the Directories field then enter the new file name in the Selection field. Alternatively, you can enter the full path and file name in the Selection field.
After selecting the new location and name of your design, click OK . You are returned to the Export dialog box and the selected path and file name appear in the field labeled New File Name (Destination) . When translated, the file name is automatically appended with suffix .iff . Note that the .iff extension is only added if the file name doesn't already contain it.
Click More Options to define the export options. The Export IFF Options dialog box appears.

Selecting Export IFF Options

This section describes the choices available in the schematic Export IFF Options dialog box.
To access the schematic Export IFF Options dialog box from the Export dialog, click More Options . The schematic Export IFF Options dialog box appears.

In the Export IFF Options dialog box, select the appropriate options for your translation using the information below.

Destination IFF File name

Use this field to specify the full path and filename for the IFF file destination. To set the directory path and filename:

Click Browse in the Export IFF Options dialog box. The Export File Selection dialog box appears.
Double-click as needed to locate the directory to place your exported IFF file in the Directories field. If a file that you want to overwrite already exists in this directory, click the filename in the Files field. Alternatively, you can append the file name to the directory path in the Selection field.
After selecting the destination for the design you want to export, click OK . You are returned to the Export IFF Options dialog box and the selected path and filename appears in the field labeled Destination IFF File name field.

IFF File Overwrite Options

Overwrite IFF File - When writing to an existing file, the contents of that file are overwritten. While this is not the default setting, it is generally the preferred setting.

Append to IFF File - When writing to an existing file, the new file is appended to the existing file. This is the default setting. The IFF file is not overwritten during the ADS export by default. To transfer multiple designs, simply use the same file multiple times. Each design is created in turn. This method enables you to transfer a limited amount of hierarchy when you don't want to overwrite reference elements. To implement this method, set the hierarchy level to None , then export one sub-network followed by the main design. No IFF data is generated for any of the referenced components in either design, so the only two circuits overwritten during an import are the two designs transferred.

Output disabled instances to the IFF file

When this option is selected, if an instance is deactivated in the schematic, it will still be output into the IFF file. If the checkbox is deselected (default), deactivated instances will not be exported. This option can be utilized to omit certain components from being transferred to remote environments that might not support the components (e.g. deactivate the simulation components prior to creating an IFF file to send to Mentor Graphics, which does not have any definitions for the simulator components). Check this option if you want to get everything. Uncheck this option if you want to filter out the unused/unwanted components.

Output ADS Item Definition properties

When this option is selected, ADS Item Definition properties are utilized to recreate the information necessary to simulate a component for ADS. For example, if you have parameters on a resistor, some Item Definition properties are created in the IFF file (e.g. R_ADS_UNIT=1), which allow the IFF importer to exactly recreate the component as it exists in ADS. However, other tools will not recognize the Item Definition parameters, and may misinterpret the properties as being separate. If library symbols are being exported to other environments that do not recognize the ADS Item Definition parameters, the option should be turned off. This option is deselected by default.

Put a space between numbers and the scalar/unit

When this option is selected, parameter values are exported as they normally appear in ADS (i.e. with a space between the number and the scalar, e.g. "1 pF"). If the checkbox is deactivated, the exporter converts the values into the IFF value specification, which is to have no space between a number and a scalar (e.g., "1pF"). Ideally, an IFF exporter should interpret either form of number, and set the value internally to whatever is normal for that environment. Some environments (e.g. Mentor Graphics) do not interpret the IFF property values in any way. For Mentor IC, this means the numbers need to have no space in them, because when they are used within SPICE simulations, the space will cause syntax errors in the simulator. However, for Mentor Board, they require the ADS components to have a space in them because the RF Architect ADS library is set up to expect values to have a space between a number and a scalar/unit.

If you are exporting designs to Mentor Boardstation, you must select this option for IFF imports to work into their environment. An additional issue can come up if you create variables, and then assign scalar values to the variable (e.g., "R1 kOhms"). When this is exported, if the option is not set, it would convert to "R1koh", which could no longer be interpreted correctly. Note that this second option is considered bad practice (the scalar should be included in the variable value for R1, and no units should be specified); however, ADS does allow you to format variables in this way. If you are using variables in this way, you must set this option to true. This option is deselected by default.

Output annotation position for schematic components

This option stores information about the position of the component text annotation in the schematic window. Annotation text includes the component type, name and parameters, as displayed next to the component. Enabling this option may be useful if the annotation has been moved in ADS. However, even with this option enabled, some environments may not preserve the position of the annotation.

Default Library Name for Library Parts

When the IFF file does not specify a library name for a component that needs to be created, the library name specified in this field is used. This is necessary for environments that do not support the concept of a library.

Design objects are stored in a group that uses the same name as the project directory, but library parts are stored in either the default library hpeesoflib or a library that you specify. The default library name can contain only alpha numeric characters.

Note
The Default Library Name For Library Parts field is identical to the field of the same name in the Import IFF Options dialog box. Changes made to this field will modify the contents of the field in the Import IFF Options dialog box.

About Component Libraries

A component library in ADS consists of a collection of component definitions. Each primitive component has an associated component name, symbol and predefined component parameters that include relevant physical and electrical characteristics.

The IFF Translator can be used as the initial step in creating an ADS component library however, this topic is outside of the scope of this manual. Creating an ADS component library using IFF requires specialized tools and training. If you're interested in learning more about this topic, contact Agilent EEsof-EDA's Solution Services.

Schematic Hierarchy Option

The Schematic Hierarchy Option drop-down list enables you to establish how much of the schematic hierarchy is exported:

Current Design Only Write current level only. Complete design information for the current design is exported. Instance-specific information (parameter values and coordinates identifying position) is also exported. Detailed definitions of a referenced design are not exported.

Current Design, Selected Projects and No Library Parts Complete design information for the current design is exported. Referenced designs that reside in a project selected for inclusion during export and are part of the current design's hierarchy are also exported. Library parts are not exported. This is the default setting.

Current Design, Selected Projects and All Library Parts Complete design information for the current design is exported. Referenced designs that reside in a project selected for inclusion during export and are part of the current design's hierarchy are also exported. In addition, library parts are exported.

Project Hierarchy

Displays the current project. If hierarchical, all included projects are listed in the appropriate order.

Projects Included During Schematic Export

This field contains the projects for which schematic design information is exported. You can customize this list if the current project is hierarchical.
To add a project to this list:

In the Project Hierarchy list, click the desired project.
Click the Include button. The project is added to the Projects Included list.
To include all projects, click Include All .

To remove a project from the Projects Included list:

In the Projects Included list, click the entry you want to remove.
Click the Remove button. The project is removed from the list.

To remove all entries from the Projects Included list, click Remove All .
This is an example of using the Project Hierarchy and Projects Included During Schematic Export fields. First you make a project called Proj_A that includes several designs. Then you make another project called Proj_B and you want to reuse some of the designs from project Proj_A in project Proj_B . You can then include Proj_A in Proj_B by using the Include button to have access to all the designs in Proj_A after your export is complete.

Completing the IFF Export

After specifying the IFF export options, click OK in the Export IFF Options dialog box to save your settings or Cancel to retain the default settings. After clicking OK , you are returned to the Export dialog box. Click OK to begin the translation.

When translation is complete, an Information Message dialog box appears stating, IFF Export Completed. The IFF Export log window also appears. Review the log message searching for any error messages or warnings generated during export.