Working with Symbols

Symbols are used to represent individual components in a schematic and subnetworks in hierarchical designs. Default symbols exist for schematics with 0 to 99 ports, but you might want to draw your own symbol for any of the following reasons:

Schematic symbols consist of a symbol body and, optionally, symbol pins (interconnect points). If you are drawing a symbol to represent an electrical component or a subnetwork for a hierarchical design, you must add pins to the symbol body.

The default symbols have been created in a uniform manner. Custom symbols should be created in a similar manner, that is, their overall length, from pin to pin, should be a multiple of 0.125 inch. This ensures the custom symbol will connect easily to the set of supplied symbols. In addition, pin 1 should be located at the coordinates 0,0 which serve as the reference point when you place the symbol in a design.

A symbol can be defined in one of two ways:

An illustration representing these differences is shown next.

For information on assigning a symbol to a schematic, refer to the section Assigning a Symbol to a Schematic.

Switching Between Schematic and Symbol Views

When you are creating a schematic, the View menu displays the command Create/Edit Schematic Symbol. When you choose this command, you display the symbol view of the current design. If you look at the View menu again, you will see that the command name has changed to read Create/Edit Schematic. This enables you to switch back and forth between these views.

If you place an instance of your schematic design as a subnetwork - without creating a special symbol - a default symbol is used, based on the number of ports in your design. If you want to create a custom symbol for your design, you can switch to symbol view and:

Refer to the following sections for details:

Creating a Symbol for use with any Design

To create a symbol for use with any design:

  1. Create a new (empty) design file.
  2. Choose View > Create/Edit Schematic Symbol.
  3. When the symbol is complete, you can associate any schematic with this symbol. For details, refer to Assigning a Symbol to a Schematic.

Generating a Symbol

You can generate a symbol for your completed schematic providing minimal specifications.

To generate a symbol:

  1. From the completed schematic, choose View > Create/Edit Schematic Symbol.
  2. In the dialog box that appears, select the Auto-Generate tab and specify the desired symbol characteristics (or accept the defaults). The symbol characteristics are defined as follows:
    Symbol Type Description
    Dual Restricts pins to two sides of symbol body
    Quad Allows pins on all four sides of symbol body
    Order Pins by Description
    Location Numbers symbol pins in the same relative order as the ports on the schematic
    Number Numbers symbol pins sequentially in a left-right, top-down order

    Replace existing symbol - Replaces the current symbol, if one exists, with the one you are about to generate.
    Lead Length - The length of any line drawn between the symbol body and a pin.
    Distance Between Pins - Distance between pins drawn on the same side of the symbol body.

  3. Click OK. A symbol is drawn consisting of a symbol body, connecting lines, and pins.

To regenerate the symbol specifying different symbol characteristics, choose Insert > Generate Symbol.

You can edit the generated symbol as desired at any time.
For details on drawing and editing shapes, refer to:

For details on symbol-specific editing, refer to:

Using One of the Supplied Symbols

You can use any of the symbols we supply and modify them or use them as is.

To associate a supplied symbol with your network:

  1. From the completed schematic, choose View > Create/Edit Schematic Symbol.
  2. In the dialog box that appears, select the Copy/Modify tab.
  3. Select the desired symbol category from the Symbol Category drop-down list and the icons for that category are displayed. These categories represent the basic component libraries, but note that not all individual components will be displayed; if multiple components share the same symbol, only one of those components is displayed.
  4. Click the desired symbol icon and its name is displayed in the Symbol name field.
    Alternatively, you can type a name directly in the Symbol name field:
    • Type an actual component name whose symbol you want to use
    • Type the name of a design file containing a symbol (or select it using the browser)
  5. Click Apply to view the symbol in the design window and click OK when you are satisfied with your symbol selection. The program compares the number of pins on the symbol with the number of ports in the schematic view and reports any discrepancies.

You can edit the supplied symbol as desired at any time.
For details on drawing and editing shapes, refer to:

Drawing a Custom Symbol

When you draw a custom symbol, you can draw it in a file containing a schematic, where it will be dedicated to that schematic, or you can draw it in an empty file and use it to represent any schematic.

Drawing Setup

Before you begin, you may find it helpful to review a number of the program's defaults, and you will most likely need to make a few changes.

Setting Snap and Grid Spacing

By displaying a grid and drawing with snap enabled, you can quickly draw objects with great accuracy. To view or change these settings, use Options > Preferences > Grid/Snap. Snap mode offers options for snapping to many different types of objects. When drawing a custom symbol, the most important option will probably be Grid, however if you are drawing complex shapes, several other options may be helpful.

The display grid can be made visible or invisible. When you turn on the grid display, you should specify a sufficiently large factor of the snap spacing so that a grid is displayed even when the snap spacing is very fine. For example, the default snap spacing (in the Schematic window) is 0.125 which means the cursor snaps every 1/8 inch. The default display factor is 2 which means that the dots appear every 1/4 inch (0.125 × 2).

Before you begin drawing, check to see if the current grid spacing is set to something other than the default of 0.125 inch; and if it is, change it back to the default and make sure Enable Snap is turned on. This step ensures that your custom symbol will easily connect to the set of supplied symbols.

Once you have drawn the symbol body and pins, you can change these settings if desired. For example, you might want to turn snap off before adding text to your design to give you more flexibility in the positioning of the text.

Specifying the Drawing Layer

All shapes and text are entered on layers. The color and visibility of any shape is controlled by the layer on which it is drawn. Before you begin drawing any part of the symbol, change the current entry layer in accordance with the part you are about to draw. For example, if you are creating a custom symbol, you should draw the symbol body, pins, and lead lines on the symbody layer so that it will be on the same layer as the supplied symbols, and subject to changes you make to that layer.

To change layers:

  1. Choose Insert > Entry Layer and a dialog box appears listing all the currently defined layers.
  2. Select a layer that is appropriate for the task at hand.
  3. Click OK. Anything you draw now is drawn on this layer. The name of the layer is displayed in the status panel of the Schematic window.

The table below lists the default layers and the types of items placed on those layers (by default).

Layer Names, Numbers, and Descriptions
Layer name Layer number Description
default 0 Objects drawn on an undefined layer are plotted on this layer. Also, if you delete a layer, any objects residing on that layer are moved to this layer.
user_symbody 1 User-created schematic symbol
user_symtxt 2 User-created schematic symbol text
user_symbol 3 User-created schematic symbol
wire 4 Wires
text1 5 Available layer name for text
labels 6 Component or item names
identifiers 7 Unique ID of components or items
parameters 8 Parameters of components or items
pin_num 9 Pin numbers and names for symbols
notes 10 Any additional descriptive information you want to add
symbody 11 Schematic symbol body outline
symdesign 12 Portion of schematic symbol contained within symbol body
SPint 13 Signal Processing integer data ††
SPfix 14 Signal Processing fixed point data ††
SPfloat 15 Signal Processing floating point data ††
SPcomplex 16 Signal Processing complex data ††
SPtimed 17 Signal Processing timed data ††
SPany 18 Signal Processing any data type ††
SPother 19 Signal Processing user-defined data ††
symtext 20 Text contained within schematic symbol body
symbodyFilled 21 Schematic symbol body with fill pattern
symbodySlash 22 The slash that identifies pin 1
The pin_num layer is visible by default, but you must turn on Pin Numbers and/or Pin Names in the Visibility (on/off) section of the Pin/Tee tab of the Preferences dialog box to make pin numbers and names appear. †† For details, refer to the information on Data Types, under the section on Data Types, Controllers, Sinks, and Components in the ADS Ptolemy Simulation documentation.

Drawing the Symbol Body

The commands you need to draw your symbol can be found on the Insert menu. In addition, many of them are available on the default toolbar. For details on using these commands, refer to Drawing Shapes under the section on Annotating Designs.

The Layer Editor dialog box enables you to determine the color and fill pattern, shape display, and line style for objects drawn on each layer.

Adding Pins to Your Symbol

There are two kinds of pins:

Symbol Pins

Remember that symbol pins should be located at 0.125-inch intervals so that your custom symbol will connect easily to the set of supplied symbols. In addition, pin 1 should be placed at the coordinates 0,0. Choose any of the methods shown below to accomplish this.

To specify 0,0 in the process of drawing pin 1:

  1. Choose Insert > Coordinate Entry and a dialog box appears.
  2. Choose Insert > Symbol Pin and a dialog box appears. Define the pin characteristics as described in the section, Establishing Pin Characteristics, and click Apply.
  3. Enter the coordinates 0,0 in the Coordinate Entry dialog box and click Apply. Pin 1 is placed at 0,0. You can now use the View All command to reposition the image in your design window.

To move 0,0 to the center of the window before you begin:

  1. Choose Pan from the View menu or the pop-up menu.
  2. Click the small cross identifying the 0,0 coordinates (lower left corner of the drawing area). The 0,0 coordinates move to the center of your design window.
  3. Choose Insert > Symbol Pin and a dialog box appears. Define the pin characteristics as described in the section on Establishing Pin Characteristics.

To move pin 1 to 0,0 after you have placed it:

  1. Choose Insert > Symbol Pin and a dialog box appears. Define the pin characteristics as described in the section on Establishing Pin Characteristics, and click Apply.
  2. Choose Edit > Modify > Set Origin.
  3. Click the pin. The pin moves to 0,0. You can now use the View All command to reposition the image in your design window.

Power Pins

Power pins, also called inherited pins, are added in symbol view, but do not appear in the schematic. They create an implied connection. This connection is inherited from subnetworks throughout the hierarchy.

There is no support for power pins in the IFF translator in the current release.

To add a power pin to your symbol:

  1. From the subnetwork design of interest, choose View > Create/Edit Schematic Symbol.
  2. If a symbol does not yet exist for the current design, the Symbol Generator appears. Set the options as desired (refer to Generating a Symbol) and click OK. A symbol is generated that includes one pin for each port of the network.
    If a symbol already exists for the current design, that symbol appears.
  3. Delete the symbol pin you want to replace with a power pin.
  4. Choose Insert > Power Pin.
    The numbering sequence for all pins of a given design must follow this rule: the symbol pin numbering sequence comes first, and the power pin numbering sequence follows.
  5. In the dialog box that appears, set the pin characteristics as needed (refer to Establishing Pin Characteristics), including renumbering, where applicable, and click Apply.
  6. Position the pointer in the drawing area and click to position the power pin.
  7. Define additional power pins for this design as needed, and click Cancel to close the dialog box.

To override the default value of a power pin for a given instance:

  1. Select the instance and choose Edit > Properties.
  2. If the instance has more than one property, select the desired property. All power properties are inherited from instances throughout the hierarchy. All properties of this type will be identified as inherited.
  3. Supply the desired Value (the name of the node or pin to which the invisible power pin should be connected).
  4. Retain the default Value Type setting of String and click OK.

Establishing Pin Characteristics

The pin characteristics are defined as follows:

To edit existing pin characteristics:

  1. From symbol view (View > Create/Edit Schematic Symbol), choose Edit > Symbol Pin or for power pins, Edit > Power Pin.
  2. Click the pin of interest.
  3. Change the settings as desired and click OK.
    When you create a symbol for use with any design, it is only available in the project directory in which you create it, unless you modify certain configuration files (and for model builder usage, modify AEL files according to stated guidelines). If you want the symbol to be available for all design work, refer to the section on Making Symbols Available Globally.

Positioning Parameters for Your Symbol

By default, when you define parameters for your subnetwork (File > Design Parameters), those parameters are positioned in the same manner as the parameters of supplied components. You can position these parameters by adding references to them using the on-screen editor in symbol view.

To position user-defined parameters for a subnetwork symbol:

  1. Open the design for which you want to customize parameter positions.
  2. In symbol view (Edit > Create/Edit Schematic Symbol), choose Insert > Text (or click the Text icon on the toolbar).
  3. Position the cursor where you want a given parameter to appear (relative to the symbol) and click once.
  4. Type the parameter name - as defined in the Design Parameters dialog box - beginning with the at symbol (@). For example, if your subnetwork has a parameter width, type @width (Parameters names are case sensitive on UNIX.)
  5. To end the text string, do one of the following:
    • Move the cursor away from the text and click once (That string is done, but the Text command is still in effect and you can click in a new location to add another string.)
    • Choose End Command (That string is done and the Text command ends.)
When using the on-screen editor to position individual parameters, do not press Enter to move from one parameter to another; you must treat each parameter as an individual text string.

When you place the subnetwork hierarchically, the parameters you positioned in symbol view appear in the same position, relative to the network symbol.

User-defined parameters positioned in this manner:

Assigning a Symbol to a Schematic

Symbols are stored in design (.dsn) files. If you generate a symbol for a particular schematic, or create one in a design file containing a schematic, then that symbol is stored in the same design file as the schematic and that symbol is automatically associated with that schematic, unless you explicitly specify the name of another symbol (design file). You can verify the symbol being used for any given schematic by opening that schematic and choosing File > Design Parameters, clicking the General tab and noting the name in the Symbol Name field. If it reflects the current design name (minus the .dsn extension), then the program will look in this file for the symbol.

If you create a symbol in its own design file-which makes it available to represent any schematic-you must assign that symbol to the desired schematic.

To assign a symbol to the schematic:

  1. Open the schematic design.
  2. Choose File > Design Parameters and the Design Definition dialog box appears.
  3. In the Symbol Name field, type the name of the file (minus the .dsn extension) that contains the desired symbol.
    The drop-down list of symbols can be modified to include any supplied symbols as well as custom symbols. For more information, refer to Modifying the List of Available Symbol Names under the section on Customization Examples in the Customization and Configuration documentation.
  4. Click OK.
    If you generate a symbol and then decide to use a custom one instead, after you type the symbol filename in the Symbol Name field, click the Save AEL button in the dialog box to save the change.
  5. Choose File > Save Design.

The next time you place this design within another design, the new symbol will appear.

To place your design within another design, select the Library Browser > Subnetworks category. Your design name should appear in the Subnetworks list.

Making Symbols Available Globally

Custom symbols are only available in the project directory where you create them unless you modify the search path of a particular variable in a configuration file. In addition, if you want the names of these symbols to appear for selection within the related dialog box, you must modify a certain AEL file.

While it is possible to leave all files containing custom symbols in the project directories in which they were created, the aforementioned configuration changes will be greatly simplified if you move all custom symbols to central locations, one location for individual use and one for site use (If necessary, see your system administrator to create the directory for site use.) We recommend maintaining the same directory structure used by Advanced Design System. Thus, the symbols should be placed in the following locations, in accordance with their use (circuit vs. adsptolemy):

Use these directories on UNIX:

Individual Use $HOME/hpeesof/circuit/symbols $HOME/hpeesof/adsptolemy/symbols
Site Use $HPEESOF_DIR/custom/circuit/symbols $HPEESOF_DIR/custom/adsptolemy/symbols

Use these directories on the PC:

Individual Use %HOME%/hpeesof/circuit/symbols %HOME%/hpeesof/adsptolemy/symbols
Site Use %HPEESOF_DIR%/custom/circuit/symbols %HPEESOF_DIR%/custom/adsptolemy/symbols
%HOME% represents the path you specified as the _Home_ _Folder_ during installation ( _C:\users\default_ by default); _%HPEESOF_DIR%_ represents the path you specified as your _Program_ _Folder_ during installation ( _C:\ADS200x_ by default).
If you use a directory other than one of those shown in the tables, then you must declare the variable USR_DSN_PATH and provide the search path.

To access custom symbols - if stored in a directory other than one of the defaults:

  1. Using any text editor, open the file $HOME/hpeesof/config/de_sim.cfg.
  2. Add the variable USR_DSN_PATH and set it equal to the path you have chosen for your symbols directory.
  3. Save the file.

Once you have created the symbols directory (regardless of where), move the files containing the custom symbols from their current project directory locations into the appropriate, newly created directory.

Modifying Search Paths

Search paths that control the order of directories searched are defined by certain program variables. These variables should be modified in a local copy of the de_sim.cfg file. This file is written to the /config directory during installation and should not be modified there. But you can open this file and copy the default variable definition (where applicable), then paste it in your own local copy and modify it (This simplifies typing a lengthy search path.)

The program creates a de_sim.cfg file automatically in $HOME/hpeesof/config. Settings modified here apply to all projects.

To modify the search path of the variable:

  1. Using any text editor, open the de_sim.cfg file in $HPEESOF_DIR/config.
  2. Locate the variable definition, copy it, and close the file.
  3. Open the de_sim.cfg file in your $HOME/hpeesof/config directory and paste the variable definition.
  4. Edit the variable definition as needed.
  5. Save the file.

Privacy Statement  | Terms of Use  | Legal | Contact Us  | © Agilent 2000-2008 

Additional Resources