Importing a Netlist File

This chapter describes the procedures for importing Spectre or SPICE netlist files into ADS using the Netlist Translator's User Interface. Performing a translation via the User Interface enables you to easily define the translation criteria and translate your netlist file. You have the option of generating either an ADS Schematic or an ADS Netlist plus an ADS Schematic with a NetlistInclude component depending on your selections.

If you have a relatively simple netlist file and only need a schematic, the ADS Schematic option is recommended. However, if you have a large or complex netlist source file or you are just more comfortable viewing a netlist version, the ADS Netlist plus an ADS Schematic with a NetlistInclude component option enables you to review the netlist. This makes it easy to compare your files line by line for debugging purposes. The netlist version also provides much faster processing.

Importing a

Importing a Netlist File Using the User Interface

Importing a netlist file to an ADS Schematic or an ADS Netlist with a NetlistInclude component using the Netlist Translator can be broken down into several simple steps.

1. Accessing the Import Dialog
2. Specifying the File Name
3. Setting the Import Options
4. Choosing the Translated Output Format
5. Defining Netlist Options *
6. Examining the Output
7. Using the NetlistInclude Component *

Note Steps 5 and 7 above are only necessary if you want to import to an ADS Netlist with a NetlistInclude component.

Creating a Simple Spectre Example

The following simple RCL-Diode circuit will be will be referred to periodically in the documentation to help with your understanding of the import process. If you like, you can create the sample Spectre file shown in Sample Spectre File (ex1.scs). You can create this file in your project directory using any ASCII text editor. Type the following text into a file.

Sample Spectre File (ex1.scs)

Save this file as ex1.scs in your current project directory then close the file. You can now use ex1.scs as an example the first time you attempt to perform an import operation.

Creating a Simple SPICE Example

Create the sample SPICE file shown in Sample SPICE File (ex1.sp). You can create this file in your project directory using any ASCII text editor. This, and other simple SPICE files, will be referred to periodically in the documentation to help with your understanding of the import process. Type the following text into a file.

Sample SPICE File (ex1.sp)

Save this file as ex1.sp in your current project directory then close the file. You can now use ex1.sp as an example the first time you attempt to perform an import operation.

Accessing the Import Dialog

You can import files through Advanced Design System's Main or Schematic window. The Import dialog box is accessed from the File pull-down menu.

Open a project in ADS before importing your design. Working in project directories enables the translator to organize design files in the standard ADS file structure.

Choose File > New Project to open a new project or File > Open Project to open an existing project.

Note The import option will not be active in the File menu unless you open a project.

For more information on working in project directories, refer to " Managing Projects and Designs " in the Advanced Design System Schematic Capture and Layout manual.

Before invoking the import procedure, close any open designs. This will remove any active designs from memory.

Choose File > Close All

To access the import dialog and import your design from the ADS Main or Schematic window:

Choose File > Import. The Import dialog box appears.

Specifying the File Name Specifying the

In the Import dialog box, choose the type of file to import, specify the filename and supply other basic information needed by the translator.

1. In the Import dialog box, select Netlist File from the File Type drop-down list if it isn't already displayed.
2. To specify the path and filename of the file you want to import, click Browse in the Import dialog box. The _
   Import File Selection_ dialog box appears.
   
3. Double-click as needed to locate the directory containing your source file in the Directories field, then click the file in the Files field. Alternatively, you can enter the full path and file name in the Selection field.
4. After selecting the design you want to import, ex1.sp for this example, click OK. You are returned to the Import dialog box and the selected filename appears in the field labeled Import File Name (Source).
5. Click More Options to define the preferred import method. The Import Netlist Options dialog box appears.

Setting the Import Options

Selecting the Dialect

In the Import Netlist Options dialog box, select the appropriate netlist dialect from the Input Netlist Dialect drop-down list.

If you are unsure of the source of the netlist file, you may be able to tell from the syntax of in line comments shown in Recognizing Netlist Variations.

Recognizing Netlist Variations

Note For HSpice, the `$' must be preceded by a space or a comma if it is not the first non-blank character because the $ is allowed within node or element names.

You may also be able to match syntax with the device table or model levels in the model tables. For more information on device and model tables, refer to Translating a Device and Translating a Model.

First line is a comment:

To make sure the first line of a source file is recognized as a comment line and ignored, the First line is a comment checkbox must be selected. This is not necessary if the line already begins with a comment character.

The First line is a comment option is available because some simulators will always ignore the first line regardless of the first character.

Use the default value for the ex1.sp example.

Suppress name mapping:

When the translator changes the name of a node or a component to comply with ADS rules, this is referred to as name mapping. Name mapping is limited to all names being changed to lowercase, as well as replacement of an illegal character with an underscore. For more information on name mapping, refer to Using Valid ADS Characters.

Click the Suppress name mapping check box to activate or deactivate this option. Activating this option enables you to override any name mapping introduced by the translator.

Note See Understanding Capitalization for cautionary information on name mapping.

Use the default value for the ex1.sp example.

Choosing the Translated Output Format

In the Import Netlist Options dialog box, there are 2 import methods available in the Translated Output Format field: ADS Schematic (with named connections) or ADS Netlist . See Translated Output Format Descriptions for format descriptions.

Note A third option, Wires , is available through the command line only. See Translated Output Format Descriptions for more information.

Translated Output Format Descriptions

• ADS Schematic (with named connections) This translation method writes an intermediate file in the Intermediate File Format (see Importing an IFF File). After the IFF file is created, it is read by ADS and the schematic is created. For detailed information on how this works, refer to Understanding the Import Operation. Components are placed in a square array and Named Connections are used to place the correct node name on each pin. Pins with the same node name are connected. This translation is faster than the Wires option that tries to connect all the pins with wires.

• ADS Netlist An ADS netlist is written to the project directory and a simple schematic is created. The schematic contains only a NetlistInclude component that references the ADS netlist file. When an ADS simulation is run, the simulator automatically reads the new netlist. This saves a lot of time on very large circuits both in translation time and simulation time, since the schematic creation and traversal are both skipped. For information on Netlist Options , refer to Defining Netlist Options. For information on editing the netlist, refer to Viewing and Editing the Netlist.

• Wires (Available from command line only) This translation method also writes an intermediate file in the IFF format. After the IFF file is created, it is read by ADS and the schematic is created. For detailed information on how this works, refer to Understanding the Import Operation. Components are placed and wired with a special algorithm. The larger the file is, the slower this will be. This method should only be used on very small circuits.

Import Methods

Caution It is highly recommended that the ADS Netlist option be used when translating large netlist file. In addition to taking many hours to create a schematic from a 20,000 line netlist, a schematic of that size is practically non-editable.

For the purpose of the ex1.sp example, select the Named Connections method and click OK in the Import Netlist Options dialog box. You are returned to the Import dialog box. Click OK to begin the translation.

Examining the Output

This section describes some of the information to look for during and after your translation to help you determine whether your translation is complete or not.

Viewing the Status Window

While the translator is running, a Status window appears and displays messages about the translation as it progresses (see Example Status Window Contents). When the translation is complete, the Status window displays the message, Translation completed, along with date and time done.

Example Status Window Contents

The Status window reports information such as the input file format, the input file name and the output format. The output format for Advanced Design System is the IFF file in this case. The translation start time is also displayed.

After the translation is complete, check to see if there were any error or warning messages reported. If any errors or warnings are displayed in the Status window, refer to Troubleshooting for information on unexpected results from the Netlist Translator and how to fix the problem.

Viewing the Schematic

Open a new schematic window and then open the ex1.dsn design to view the schematic. For more information on schematic windows, refer to "Working in Design Windows" in the ADS Schematic Capture and Layout manual.

ADS Schematic Window with Translated ex1.dsn.

Before simulating your design in ADS, you will need to place simulation control blocks from one of the simulation palettes in the schematic window. You may also need to place an instance of an imported design in a new schematic. For more information on setting up your simulation, refer to Simulating the Translated Netlist.

Defining Netlist Options

If you selected ADS Netlist in Choosing the Translated Output Format, the Optional Directory Location area of the Import Netlist Options dialog is activated. Specify the component name (use all lower case), number of pins and an output directory in each of the respective fields, according to the guidelines below.

• Directory to Store Netlist To specify the path of the directory you want to store your netlist in, click Browse. The Netlist Directory Selection dialog appears. If you do not choose a directory to store your netlist, it will default to your current project directory.

• Element Replacement Table If you created a custom component in Advanced Design System that you want the system to use when it imports a netlist in place of the default ADS component, see Using a Custom Component for instructions on completing this field.

Once all options are entered, click OK. You are returned to the Import dialog box.

Click OK on the Import dialog box. The following informational dialog appears:

The informational dialog informs you that you have selected an ADS netlist import and that you will need to select a subcircuit from your netlist to be the top level circuit that will used for the simulation.

Click OK on the informational dialog to select the subcircuit. The following dialog appears:

All of the existing subcircuits with their pin counts are listed.

Note Only the subcircuits from the Spectre or SPICE netlist that you entered in the Import dialog are listed. If you want to use a subcircuit that is contained in an include file, you have to manually add that after the import process is complete.

Select the subcircuit to use as the top level subcircuit and click OK to start the translation.
The Netlist Translator performs the automatic translation of your source file into an ADS Netlist plus an ADS Schematic with a NetlistInclude component (see ADS Schematic Window with NetlistInclude Component.).

ADS Schematic Window with NetlistInclude Component.

Viewing and Editing the Netlist

If you selected ADS Netlist in Choosing the Translated Output Format, the Netlist Translator creates an ADS netlist and places it in the project directory. The ADS netlist is in the form filename .net, where filename is the component name you specified in the Import Netlist Options dialog box.

To view and edit the netlist, open the ADS text editor from the Main window, Tools > Text Editor . You can also view the netlist from a command shell or with any ASCII text editor. Translated ADS Netlist (ex1.net) displays the translated ADS Netlist, ex1.net , of the example file, ex1.sp.

Translated ADS Netlist (ex1.net)

Once you have your netlist displayed, verify that the translated netlist and the original netlist have the same parameters. For more information on parameter mapping in devices and models, refer to Translating a Device and Translating a Model.

Using Imported Designs in ADS

This section provides additional information that can help you prepare for simulating your imported designs in Advanced Design System. Depending on your specific needs and the way your translation was performed, you may be required to perform these steps before your design can be simulated. For information on simulating your design, refer to Simulating the Translated Netlist.

Checking for Unconnected Nodes

If the log file reported any components that could not be translated, there will be open connectors which show up as red diamonds on the pins in the schematic. Pins that have a red diamond when the schematic is complete are not connected to any other pins. To check for unconnected nodes on a large schematic where the red diamonds are hard to see:

1. From the schematic window, choose Options > Check Representation . The Check Representation dialog box is displayed.
2. Ensure the Unconnected pins check box is active and then click OK . A Check Representation Report is displayed that will list all unconnected pins. Note that the components with unconnected pins are highlighted on the schematic.
3. In the Check Representation Report , click Print to save the report to a file. Click OK to clear the dialog.
4. To clear the highlighted components on the schematic, choose Layout > Clear Highlighted > Components .
   If a pin is not connected, it may be because the component it was connected to was not included in the original file. More likely, the translation of that component failed because of a syntax error or there is no equivalent ADS component. In this case, you should manually place a component and connect them using the Insert > Node Name command.

A message will be written to the translation log file (nettrans.log) in the case of any failures. For more information on the translation log, refer to Viewing the Translation Log.

Note There is no visible indication of unconnected nodes in the output ADS Netlist, so the log file must be checked for the names of un-translated components.

Including Models and Subcircuits

This section describes how to include models and subcircuits in your existing design using several example files. Before continuing, create the two example files shown in Transmission Line Subcircuit (tline.sp) Netlist and Transmission Line Inverter (inverter.sp) Netlist. Save each of the files in the project directory that was used for storing the example SPICE netlist (ex1.sp) in Accessing the Import Dialog.

The two new example SPICE files make up a simple transmission line inverter. The first SPICE netlist (tline.sp) is a subcircuit.

Transmission Line Subcircuit (tline.sp) Netlist

The next SPICE netlist (inverter.sp) includes additional components that complete the transmission line inverter design.

Transmission Line Inverter (inverter.sp) Netlist

Import both of your new SPICE files individually using the information in Importing a Netlist File Using the User Interface. These two files should be imported using the PSpice dialect and the Named Connections import method. Remember to close all designs before starting each import.

After the designs have been imported, leave the design inverter.dsn open. Notice the red diamonds on this schematic indicating that something is missing from the file. In some cases, this is caused by components that could not be translated (see Checking for Unconnected Nodes). In this case however, the original SPICE file did not supply this component so the tline.dsn subcircuit will be used to complete the circuit.

Including a Subcircuit

Your SPICE netlist may contain one or more subcircuit definitions. A subcircuit in the SPICE file becomes a reusable component in the ADS schematic. To use a subcircuit, you can place an instance of it in a new or existing design.

To browse for a component and include it in your design:

1. From the schematic window, choose Insert > Component > Component Library or click the Display Component Library List button on the toolbar.

   The Component Library/Schematic dialog box is displayed.

2. In the Libraries field, scroll down in the list until you find either the Spice Netlists library or the Sub-networks library.
3. Click either the Spice Netlists library or the Sub-networks library in the Libraries field to see the list of subcircuits that can be placed as components.
4. In the Components field, click the Component that you want to use ( tline in the example case) and move the cursor back into the schematic window.
5. Click to place the component in your schematic.
6. Click the End Command And Return to Select Mode icon from the tool bar to stop placing instances of your component.

If you know the name of the subcircuit without looking it up, you may type it directly into the Component History drop-down list box as illustrated below.

When you enter the name of the subcircuit in the component history box, the case must match exactly with the design name in ADS. Your subcircuit name will be all lower case unless you checked the Suppress name mapping option in the Import Netlist Options dialog box. For more information on capitalization and name mapping, refer to Understanding Capitalization and Suppress name mapping:

Note If your SPICE netlist contains a set of models outside of any subcircuit block, the models will be placed in a separate top level design that has the same name as the SPICE file. To use these models, copy them into the design that references them. Optionally, a design with models only can be placed as a subcircuit within another design, but all of the models have to be edited to have global scope. To do this, select a model, open the edit parameter dialog, click the Component Options button and change Scope to Global .

Example Spectre Subcircuit with Referenced Parameter Value

The following example illustrates a translation of a Spectre subcircuit into an ADS netlist. The Spectre subcircuit contains two parameters with default values. The value of the second parameter, r2 , refers to the first parameter, r1 . (The value of r1 could either be the default value or a specified value when the subcircuit is called from an instance component.)

ADS does not directly support parameter default values that reference values of other parameters passed into the subcircuit. Using the backward compatible option (-bc), the Netlist Translator manages this by placing extra variables (in this example, ADS_r2_1, ADS_r2_2, and UNDEF) and an equation(s) within the netlist to calculate the correct value of the contingent parameter (in this example, r2 ). Without the -bc option, ADS will read the subckt statement with parameter referencing in Spectre syntax. Thus the subckt header is wrapped with the lines simulator lang=spectre and simulator lang=ads.

Note Tnom is added by default to resistor component to match Spectre simulation results. This is done only when no Tnom parameter is set.

Note This is only available through the command line. Use the -pp (preserve parameter) option.

Spectre subcircuit

subckt myexample \(t1 t2 s\)
parameters r1=1 r2=r1
R0 \(t1 net1\) resistor r=r1
R1 \(net1 t2\) resistor r=r2
ends myexample

ADS subcircuit-translated in backward compatibility mode (using -bc option)

define myexample \(t1 t2 s\)
parameters r1=1 r2="UNDEF"
ADS_r2_0=r1
ADS_r2_1=if \(r2 == "UNDEF"\) then ADS_r2_0 else r2 endif
R:R0 t1 net1 R=r1 Tnom=27
R:R1 net1 t2 R=ADS_r2_1 Tnom=27
end myexample

ADS subcircuit-translated in default mode (without using -bc option)

simulator lang=spectre
subckt myexample \(t1 t2 s\)
parameters r1=1 r2=r1
simulator lang=ads
R:R0 t1 net1 R=r1 Tnom=27
R:R1 net1 t2 R=r2 Tnom=27
end myexample

Connecting a Component

This section describes how to set pin number preferences and assign node names in order to connect a subcircuit to a design. After placing the instance of the Transmission-Line Inverter subcircuit in the last example, you can use the ADS Node Names to connect the subcircuit pins to the rest of the circuit. You may need to turn the pin number visibility on to help identify the proper pins when naming nodes.

To set the Pin Numbers schematic preference in order to see the pin numbers:

1. From the schematic window, choose Options > Preferences . The Preferences for Schematic dialog box is displayed.
   
2. Select the Pin/Tee tab.
3. Click the Pin Numbers check box in the Visibility (on/off) section to activate the pin number visibility.
4. Click OK to save the settings and close the dialog box.

Defining the Node Names

To define the node names to connect the subcircuit:

1. Choose the Insert > Wire/Pin Label menu selection or click the Insert Wire/Pin Label icon in the tool bar.

   The Wire/Pin Label dialog box appears.

   

2. Enter n2 in the Node Name field but DO NOT click the Done button. An instance of n2 is attached to your cursor.
3. Drag your cursor onto the schematic and click pin 1 of the subcircuit symbol.
4. In the Node Name dialog box, change the node name to n4 . Again, DO NOT click the Done button. Drag your cursor onto the schematic and click pin 2 of the subcircuit symbol.
5. Save your new design as tline_inv.dsn.

This completes the circuit. Your combined inverter.dsn and tline.dsn should now appear similar to the tline_inv.dsn schematic design shown in Translated_Schematic_with_Subcircuit_(tline_inv.dsn)._This_design_is_used_in_the_simulation_example_in_Simulating the Translated Netlist.

Translated Schematic with Subcircuit ( tline_inv.dsn )

Creating a Hierarchical Project

You can create hierarchical projects using the Include/Remove Projects command. This command creates a reference, or link to another project.

If the import has produced a set of models or subcircuits that will be maintained in a project directory other than the one a designer will be working in, that project directory should be included into the working project directory so the simulator can see the imported items. The Include & Remove dialog can be accessed from the Main window. To include a project directory:

1. Open the working project directory from which you want to reference designs in other projects.
2. From the Main window, choose File > Include/Remove Projects. The Include & Remove dialog appears.
3. Use the File Browser to locate and select the project you want to include. This would be the project containing the set of models or subcircuits.
4. Click the Include button. The project is added to the Project Hierarchy listing.
5. Repeat as needed, then click OK.

Using the NetlistInclude Component

If you selected ADS Netlist in Choosing the Translated Output Format, your translated schematic will contain a NetlistInclude component. This section describes how you can view and modify the NetlistInclude component and then use the component within another design.

The NetlistInclude component in this section is created by modifying and translating a previous example SPICE Netlist into an ADS Netlist with a NetlistInclude component. The newly translated design is then used to show how you can place an instance of your NetlistInclude component into another design and then simulate the design.

To setup and translate your example SPICE Netlist into an ADS Netlist with a NetlistInclude component:

1. Close any open designs. Choose File > Close All.
2. If it's not already opened, open your project that you created in [ "Importing a Netlist File Using the User Interface" |Importing a Netlist File#1106823]. Choose File > Open Project.
3. From the ADS Main window, choose Options > Text Editor to open the ADS text editor.
4. In the text editor, choose File > Open and open the file tline.sp that you created in Transmission Line Subcircuit (tline.sp) Netlist in Including Models and Subcircuits.
5. Choose File > Save As to save the file with a new name, tline2.sp.
6. Edit the new file to change the subckt name to TLINE2 as shown in the following table, then re-save and close the new file.

   *TRANSMISSION-LINE SUBCIRCUIT .SUBCKT TLINE2 1 3 T1 1 2 3 4 Z0=50 TD=1.5NS T2 2 0 4 0 Z0=100 TD=1NS .ENDS TLINE .END

7. From a blank schematic window, import the new file tline2.sp . In the Import Netlist Options dialog box, select PSPICE as the Spice Dialect and ADS Netlist as the Connection Method For Schematic. If you need more information on importing a SPICE file, refer to Importing a Netlist File Using the User Interface.
   
8. Click OK to exit the Import Netlist Options dialog box.
9. In the Import dialog box, click OK to translate the netlist. An information dialog appears that informs you to select a subcircuit that exists within the netlist.
   
10. Select the tline with 2 pins from the Netlist Subcircuit List dialog box and then click OK.
    Once your translation is complete, ADS displays a schematic window with the tline2.dsn that contains two ports and a NetlistInclude component similar to the one in the following illustration.
    

    Design Containing Two Ports and a NetlistInclude Component

11. Note that the File parameter in the NetlistInclude component is called tline2.net. The translated file tline2.net is now in the project directory and looks like the netlist in the following table. You can use the ADS text editor to open and view the ADS Netlist.

Translated Transmission Line Subcircuit (tline2.net) Netlist

To view the design details of your NetlistInclude component:

1. From the schematic window, choose File > Design Parameters. The Design Parameters dialog box appears. The General tab is displayed by default.
   
   • The Name and Description fields display the current design name by default.
   • The Component Instance Name field default is X. The text in this field is used as a prefix in building a unique name (ID) for every item. This prefix becomes part of the annotation displayed with the symbol representing the parametric subnetwork when you place it in a design.
   • The Symbol Name field displays the standard symbol with the number of ports that you specified for the circuit in the Import Netlist Options dialog.
   • The Library Name field displays the name of the library that the design is owned by. This might be something like Spice Netlists. For more information, refer to Including Models and Subcircuits.
2. Click the Parameters tab. The Parameters tab does not apply to this particular example; however, you may find it helpful to understand the function of this dialog box for future reference.
   
   When you import a SPICE file containing a subcircuit with parameters to an ADS schematic, you can use this tab to view or edit the parameter details. Each parameter is listed in the Select Parameter field and has characteristics that determine how it is handled when the network is reused. These include the Parameter Name , the Value Type assigned to the parameter, the Default Value , and optional control attributes. Default values are listed only if they were specified in the SPICE file.
   For more information on subcircuit parameters, refer to ".SUBCKT"]. For more information on using the Design Parameters dialog, refer to "Defining Parameters" in the ADS Schematic Capture and Layout manual.
3. Click OK to continue.

To add an instance of your imported design:

1. Open the schematic tline_inv.dsn that was created as a result of Including Models and Subcircuits and shown in Translated Schematic with Subcircuit (tline_inv.dsn).
2. Save the tline_inv file as tline_inv2.dsn using the File > Save As command.
3. In the tline2_inv schematic design, delete the tline component.
4. In this example, tline2 is the imported design with the NetlistInclude component. An instance of this component can be placed in your tline_inv2 design by entering the name tline2 in the component history box. This attaches an instance of the component to your cursor that you can now click into place. Place the instance of tline2 in an appropriate location on the tline_inv2 schematic.
   
5. Connect the appropriate circuitry to the new subcircuit by naming pin 1 n2 and pin 2 n4 . For more information on naming nodes, refer to Defining the Node Names.
6. This completes the circuit. This circuit can now be simulated using the example shown in Simulating the Translated Netlist.
7. ADVANCED OPTIONS

You may create your own symbol by drawing it in the symbol view ( View > Create/Edit Schematic Symbol ) and changing the Symbol Name in the Design Parameters dialog to the name of the design, tline2 in this example. Save the AEL file from the Design Parameters dialog and the design file from the File menu. A new symbol will not automatically appear in the design in which it is used. For the new symbol to appear in your design, replace the instance of tline2 in your test circuit.

For additional information about the NetlistInclude component, refer to Adding the NetlistInclude Component.

Understanding Import Details

This section describes some of the unique details of the translation process that should be understood before attempting to translate a design.

Using Valid ADS Characters

The legal character set for Advanced Design System names is alphanumeric _ + - = ^ ' @ # & $ %. Legal characters other than alphanumeric and underscore require special handling. Any string using special characters in ADS must be enclosed by quotes. This is handled by the translator.

Note Do not insert extra quotes in your file. Additionally, $ and % are not allowed in subcircuit names since these become invalid design and file names.

If the translator encounters an illegal character (any character not listed above), the illegal character is replaced with an underscore and a warning message is written to the log file.

Understanding Capitalization

Like Spectre, ADS is a case sensitive system, so Abc and ABC represent two different designs, components, etc. If the Suppress name mapping option is not selected in the Import Netlist Options dialog, the translator converts all node names, element and model names, variable names and subcircuit names to lower case. Conversion to all lower case can cause a problem if the design being imported references an existing ADS design that has a mixed case name or a name that is all capitals. In addition, this can case a problem if two or more items are referenced within the Spectre netlist use case to differentiate between them, for example, two components named RS and rs.

Refer to Suppress_name_mapping:_for_information_on_toggling_the__Suppress_name_mapping__option._For_more_information_on_the_command_line_option,_refer_to_Importing a File from the Command Line. If this option is used, the names in the file must use consistent capitalization; for example, every time Abc is used, it must be capitalized the same.

Using Unique Names

The Spectre and SPICE simulators are less restrictive than ADS with regards to unique names. Model names must be different than device names and the translator modifies the device name to help provide uniqueness.

The only other restriction is that a subcircuit cannot override the name of a built-in component. The translator does not check for this at this time, since the library of parts is always growing and the translator is run as a separate process from ADS.

• On UNIX, this should not be an issue because component names in ADS typically begin with a capital letter, and any subcircuit name that is output by the translator will be in lower case. The exception would be if the Suppress name mapping option were turned ON. For more information on the Suppress name mapping option, refer to Suppress name mapping:.

• On a PC, this may present a problem in ADS because design names follow a case-insensitive rule (for this one particular case). Because design names become file names and the file system is case-insensitive, a subcircuit could potentially attempt to override a built-in component.
  If there is a situation where the name of the subcircuit is the same as the name of an existing ADS component, the name of the subcircuit will be changed in the schematic created by the translator. This will not be the case if the netlist option is used, which will lead to an error during simulation. The user is responsible for unique names in this situation.

Using Global Nodes

Global nodes are node names which, when used at any level of the hierarchy in the circuit, will be connected to the same node. In Spectre, you declare a global node in the following manner in a definition statement (the first node is always assumed to be ground):

global gnd VCC1 VCC2

or

gnd! VCC1! VCC2!

Berkeley SPICE does not support global nodes and HSpice and PSpice have different implementations. In HSpice, a global node in a definition statement is declared as:

.global VCC1 VCC2

In PSpice, it is just defined when used by putting $G_ in front of the node name:

$G_VCC1 $G_VCC2

Global nodes are translated in the style of PSpice except that instead of special characters at the beginning, an exclamation point is appended to the node name when it is used. In the example above, the node names become VCC1! and VCC2!. Additionally, this must be quoted since the exclamation point is a special character to ADS, so it becomes "VCC1!" and "VCC2!".