Creating Elements

This topic presents details for creating new items in Advanced Design System (ADS).

Creating New Items

There are two basic categories of items that can be placed in a design: items that can be simulated and items that cannot be simulated. Simulated items, include all the program-supplied items in the libraries and palettes and all user-defined networks. Non-simulated items, are termed objects. Typical objects are alignment markers, schematic sheet borders, mechanical fasteners, etc. Objects can be selected from palettes and libraries like any other item, but are not included in simulation, nor are they normally included in design synchronization between layout and schematic.

Simulation Items

Simulation items, as the name implies, are included in simulation. Each simulation item has one of two types of simulation models associated with it: models represented as schematics and built-in simulation models. Either type can be used when creating a new item. Built-in models can be user-defined items, or any item for which the simulator has an intrinsic representation. For more information on creating user-defined elements, refer to the User-Defined Models or ADS Ptolemy Simulation documentation.

Creating a new item using a built-in simulation model can be used to assign artwork to items with no default artwork assignment, such as lumped components or device models. An example application would be to create a new item for a FET that is modeled with an S-parameter file using the S2P item.

Creating a new item modeled with a schematic network allows a greater degree of freedom. An example would be creating a network that models the parasitic effects of the solder pads for a Surface Mount Technology (SMT) lumped component. The ability to pass parameters into custom networks increases the flexibility of this approach by allowing any network to be parameterized in the same manner as built-in simulation models.

Defining a New Item

You can define any type of new item by selecting File > Design Parameters from the Schematic or Layout window. Filling in the fields of this dialog box creates a custom item definition.

The custom item definition is stored in an AEL file. This file is named <design>.ael, where design is the name of the open design file. This file contains a number of AEL function statements. These functions register the new item with the Design Environment. This registration includes which palettes and libraries the item should show up in, how the item will be simulated (if at all), what the item's parameters are, the item's artwork and other details. It is possible to view and edit this AEL file using a text editor (the syntax for these functions is defined in the AEL manual). However, the syntax is complex and using the dialog box eliminates many possible errors in defining a new item.

Once the item definition is complete, the item can then be placed and used in your designs in the same manner as those supplied by the program. By default, your custom items are assigned to the Subnetworks directory of the current project, but you can store it in a library of your own choosing by supply a new library name.

If you are creating an item with a schematic network model or an item using custom artwork, you should create the network or artwork before creating the new item definition. For items using a schematic network, the item definition is usually done with the completed schematic network open in the Schematic window. For any other type of item definition, the Schematic and Layout windows are usually empty. The artwork and models are in other design or AEL files and are referenced by name.

Defining Design Characteristics

While the default design characteristics may be acceptable in many cases, the Design Parameters dialog box allows you to alter the default characteristics of the network. You may want to modify any or all of the following default characteristics founder on the General tab.

Name - This field is informational only and displays the current design name.

Description - Provide any descriptive phrase for clarification. This description appears in the Component Parameters dialog box when placing the item or network.

Component Instance Name - The default is X, but 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 when you place it in a design.

Symbol Name - The filename you supply in this field specifies the symbol used when you place the item in a design. You can supply a symbol name in one of several ways:

• You can type the desired name here. If you type a filename, it must be the exact filename (minus the .dsn extension) of any file containing only a symbol.
• You can select a symbol from the list of symbols on the drop-down list. This list contains several common symbols available by default. You can add to this list the names of any symbols you have created by adding the filenames to the list through AEL. For details on how to do this, refer to the section Modifying the List of Available Symbol Names under the section on Customization Examples in the Customization and Configuration documentation.
• Click More Symbols to bring up a dialog box that displays icons for all supplied symbols.
  When you specify a symbol, make sure that it has the correct number of ports.

Library Name - By default this field contains an asterisk (*) and if you accept this default, your item will be stored in the Subnetworks directory of the current project. This name can be changed to any custom-defined library name.

Allow only one instance - This enables you to specify whether or not the item or network can be placed in a design more than once. The default is off, meaning the item or network is not unique and can appear more than once in a design. Change to on if you want to restrict placement to once per design.

Include in BOM - Turn this on if you want the details of the subnetwork design to be included in a generated Bill of Materials (BOM). When this is turned off, only the top level design information is included.

Layout Object - Turn this on if the design you are defining is an object used with the Layout option (Layout objects are not simulated or synchronized but typically contain items such as alignment markers.) This attribute controls whether or not they will show up in layout palettes and libraries or schematic palettes and libraries.

Simulate From Layout (SimLay) - Analog/RF designs only. The netlist required for simulation is generated from either the Schematic or the Layout. Select this option to generate the netlist from the Layout.

Simulation

• Model - Enables you to assign a netlist choice:
  • Built-in Component - A built-in simulator item (such as CAP or RES)
  • Subnetwork - A schematic network you have defined
  • Not Simulated - Create layout or schematic only non-simulated items
• Simulate As - This field should contain the name of a built-in simulator item or the name of a schematic (usually the name of the current design). If the Simulation Model is set to Subnetwork, enter the design name; if it is set to Built-in Component, enter the name of a built-in simulator item or select one from the drop-down list. If you chose Not Simulated for the item, this field is unused.

Artwork

• Type - Enables you to assign an artwork type: Synchronized, Fixed, AEL Macro or None.
• Name - Enables you to assign a macro item or design item with the appropriate artwork name.

Save AEL File - Enables you to incrementally save definitions (which are contained in the .ael file). By turning this on and choosing OK, rather than waiting until you save the design file itself, the AEL definition for the new item is saved.

If the default design characteristics meet your needs, you can proceed directly to the section on Defining Parameters.

Creating a New Item Using a Built-in Simulator Model

To define the simulation model, first create a new empty design using File > New Design in the Schematic window. Define your design characteristics and add any parameters that need to be passed to your item (File > Design Parameters). Once the parameters are defined, save the item definition.

For the following topics discussed in this section, you will be using a simple capacitor CAP as the simulation model, with predefined artwork representing a chip capacitor footprint CHPCAP.

To define an item using a built-in model:

1. Create a new project or open an existing project.
2. Open a Schematic window and select File > New Design.
3. Give the file a name (in this example, mycap).

   Note You do not need to place anything in the Schematic or Layout windows for this example-the entire item definition is done through the Design Parameters dialog box.

4. Choose File > Design Parameters. The Design Parameters dialog box appears.
5. Optionally, enter a new Item ID Prefix for your item, in this example, C.
6. Specify a Symbol Name using one of the methods described earlier. In this example, the supplied capacitor symbol, SYM_C, is used.
7. Enable the Layout Object option.
8. Specify an Artwork Type, for example Fixed.
   When you design a network, you need to determine what type of artwork should represent your network when it is placed in another network. For creating most elements, either Fixed or AEL Macro should be used.
9. Specify a name in the Artwork Name field (for fixed artwork, enter the same name that appears in the Label field; for a macro, enter the name of the AEL function). For this example, select CHPCAP as the artwork for a chip capacitor.
10. Select the appropriate simulation model, as described earlier. In this example, use Built-in Component.
11. Specify how you want the item (or network) simulated. Select C for this example. Your dialog box should now look like the following example.
    
12. Click Save AEL to save this portion of the item definition, and continue to the next section, Defining Parameters.

Defining Parameters

Most new items you define need parameters. In this example, the parameters for the new item are the same as those for the Simulation Model, CAP, i.e., C (capacitance). For items with AEL artwork, you may need to add additional parameters (at the beginning of the parameter list) for layout.

In this example, the first artwork, CHPCAP, has no additional parameters for layout, so you only need to define the parameter C for this item. After selecting Built-in Component as the model type, you can click on the Parameters tab to define parameters.

Hint You can click Copy Component's Parameters and the set of parameters for the item named in the Simulate As field (in this example, CAP) is assigned automatically to your new item. In this example, this is the only step needed to define parameters, since there are no extra layout parameters.

For more complex definitions, each parameter has characteristics that determine how it is handled when the item is used. These include the name and label displayed in the Component Parameters dialog box, the unit type for the parameter, the type of value assigned to the parameter, the default value, and certain control attributes.

To define a parameter:

1. For this example, click Copy Component's Parameters then click the Parameters tab. The parameters for the supplied capacitor component are listed.
   

   Important For AEL generated artwork, entering your parameters in the correct order is critical. The order you specify in this dialog box must match the order given in the function. For example, in the AEL function for an MLIN, width comes before length. If you enter the length parameter first, it is still read by the function as width (ignoring the Name identifier). Also, artwork parameters must precede those used for simulation, and must be marked Not Netlisted. For items with artwork, add any artwork parameters first, then use copy parameters or add the simulation parameters.

2. In this example, since parameters of a supplied component were copied, the Edit Parameter fields are filled in with defaults.
   • The Value Type is set to Real.
   • The Default Value is set to 1.0 pF. Note that this value serves only as a default. You can change the value each time you place the item subsequently.
   • The Parameter Type is set to Capacitance.
   • The Parameter Description (optional) reads Capacitance (This is used only to document the meaning of the parameter.)
3. Enable or disable the following options, based on your design needs:
   • Display parameter on schematic - Select this option to display, on the schematic, the parameter being defined.
   • Optimizable - Select this option to allow this parameter to be optimized.
   • Allow Statistical Distribution - Select this option to allow post-production tuning for this parameter during yield analysis.
   • Not edited - Select this option to prevent this parameter from appearing in the Component Parameters dialog box for editing and always use the default value assigned here instead.
   • Not netlisted - Select this option to prevent a parameter from being considered in simulation, but still be recognized for artwork generation. (In general, layout-only parameters - not used for simulation - are assigned the Not Netlisted attribute.)
4. If defining new parameters (as opposed to copying the simple parameters for this example), you must click Add to add each new parameter to the parameter list.

   Hint You can assign attributes for each parameter as you define it, or you can define all parameters and then go back and assign attributes.

5. Save your design.
   When the design file is saved, an AEL definition is created in the /networks directory of the current project. This file (along with the design file containing the schematic/layout) can then be moved to other directories for use as library parts, either for personal use or site-wide use. For details, refer to Creating Custom Libraries under the section on Customization Examples in the Customization and Configuration documentation.
   For details on adding items to a palette, see the de_define_palette_group() function in the AEL documentation.