PSpice Schematics Schematic Capture Software User’s Guide
Copyright © 1985-2000 Cadence Design Systems, Inc. All rights reserved. Trademarks Allegro, Ambit, BuildGates, Cadence, Cadence logo, Concept, Diva, Dracula, Gate Ensemble, NC Verilog, OpenBook online documentation library, Orcad, Orcad Capture, PSpice, SourceLink online customer support, SPECCTRA, Spectre, Vampire, Verifault-XL, Verilog, Verilog-XL, and Virtuoso are registered trademarks of Cadence Design Systems, Inc.
Contents Before you begin xv Welcome . . . . . . . . . . . . How to use this guide . . . . . Symbols and conventions Related documentation . . Chapter 1 Chapter 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xv . xvii . xvii xviii Overview . . . . . . . . . . . . . . . . . . . . . . . . . . Using PSpice Schematics . . . . . . . . . . . . . . . . . Example—Drawing a Schematic . . . . . . . . . . . . . Starting a New Design . . . . . . . . . . . . . . .
Contents Chapter 3 Using the Schematic Editor 27 Overview . . . . . . . . . . . . . . . . . . . . . Components of a Design . . . . . . . . . . . . . Parts . . . . . . . . . . . . . . . . . . . . . . Symbols . . . . . . . . . . . . . . . . . . . . Ports . . . . . . . . . . . . . . . . . . . . . . Attributes . . . . . . . . . . . . . . . . . . . Annotations . . . . . . . . . . . . . . . . . . Connections . . . . . . . . . . . . . . . . . . Main Window . . . . . . . . . . . . . . . . . . Menus . . . . . .
Contents Opening a File . . . . . . . . . . . . . . . . . . . . Finding Parts . . . . . . . . . . . . . . . . . . . . . . . Getting Parts by Name . . . . . . . . . . . . . . . Searching for Parts in the Libraries . . . . . . . . Placing and Editing Parts . . . . . . . . . . . . . . . . Rotating and Flipping Parts . . . . . . . . . . . . Editing Part Attributes . . . . . . . . . . . . . . . Global Editing of Attributes . . . . . . . . . . . . Editing the Default Attributes of a Symbol . . . .
Contents Printing Your Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140 Scaling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 Closing the Schematic Editor . . . . . . . . . . . . . . . . . . . . . . . . . 146 Chapter 5 Using the Symbol Editor 147 Overview . . . . . . . . . . . . . . . . Components . . . . . . . . . . . . . . Symbols . . . . . . . . . . . . . . . Packaging Information . . . . . . Footprints . . . . . . . . . . . . . . Simulation Models .
Contents Making a Copy of a Symbol . . . . . . . . . . . . . . . Importing a symbol definition . . . . . . . . . . . . . . Using AKO Symbols . . . . . . . . . . . . . . . . . . . Drawing Symbol Graphics . . . . . . . . . . . . . . . . . . Elements of a Symbol . . . . . . . . . . . . . . . . . . . Selecting . . . . . . . . . . . . . . . . . . . . . . . . . . Filling Shapes . . . . . . . . . . . . . . . . . . . . . . . Ordering Drawing Objects . . . . . . . . . . . . . . . . Rotating and Flipping Elements .
Contents Setting Up Multiple Views . . . . . . . . . . . . . Translators . . . . . . . . . . . . . . . . . . . . Navigating Through Hierarchical Designs . . . . Assigning Instance-Specific Part Values . . . . . . Passing Information Between Levels of Hierarchy Example—Creating a Hierarchical Design . . . . Drawing the Top-Level Schematic . . . . . . . Drawing the Lower-Level Schematic . . . . . Chapter 8 Chapter 9 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Contents Setting Package Class Priorities . . . . . . . . . . Generating a Bill of Materials Report . . . . . . . . . Printing and Saving the Report . . . . . . . . . . Customizing the Format of the Report . . . . . . User Defined Component Information . . . . . . Exporting to a Spreadsheet or Database Program Swapping Pins . . . . . . . . . . . . . . . . . . . . . . Interfacing to Board Layout Products . . . . . . . . . Layout Mapping Files . . . . . . . . . . . . . . . . Back Annotation . . . . . . . . .
Contents Glossary Index x 331 337
Figures Figure 1 Figure 2 Figure 3 Figure 4 Figure 5 Figure 6 Figure 7 Figure 8 Figure 9 Figure 10 Figure 11 Figure 12 Figure 13 Figure 14 Figure 15 Figure 16 Figure 17 Figure 18 Figure 19 Figure 20 Figure 21 Figure 22 Figure 23 Figure 24 Figure 25 Interaction of Sim Software Programs and Files . . . . . . . . . . . . Opto-isolated, Addressable Serial-to-parallel Converter Circuit . . . Border Styles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Figures xii
Tables Table 1 Table 2 Table 3 Table 4 Table 5 Table 6 Table 7 Table 8 Table 9 Table 10 Table 11 Table 12 Table 13 Table 14 Table 15 Table 16 Remaining Parts to be Placed . . . . . . . . . . Standard Schematics Toolbar . . . . . . . . . . Drawing Toolbar . . . . . . . . . . . . . . . . . Simulation Toolbar . . . . . . . . . . . . . . . Annotation Graphics Toolbar . . . . . . . . . Schematic Editor Function Keys . . . . . . . . Zoned Border Default Decimal Parameters . .
Before you begin Welcome Orcad family products offer a total solution for your core design tasks: schematic- and VHDL-based design entry; FPGA and CPLD design synthesis; digital, analog, and mixed-signal simulation; and printed circuit board layout. What's more, Orcad family products are a suite of applications built around an engineer's design flow—not just a collection of independently developed point tools. PSpice Schematics is just one element in our total solution design flow.
Chapter Before you begin • graphically characterize simulation stimuli using the fully integrated PSpice Stimulus Editor, so stimulus definitions are automatically associated with the appropriate symbols • graphically characterize simulation models using the fully integrated PSpice Model Editor utility, so model definitions are automatically associated with the appropriate symbols • interface to PSpice Optimizer for analog circuit performance optimization • interface to PCB programs for printed cir
How to use this guide How to use this guide This guide is designed so you can quickly find the information you need to use PSpice Schematics.
Chapter Before you begin UPPERCASE In Capture, open CLIPPERA.DSN. Path and filenames are shown in uppercase. In the example, you open the design file named CLIPPERA.DSN. Italics In Capture, save design_name.DSN. Information that you are to provide is shown in italics. In the example, you save the design with a name of your choice, but it must have an extension of .DSN.
How to use this guide This documentation component . . . Provides this . . . Orcad family customer support at www.orcad.com/technical/technical.asp An Internet-based support service available to customers with current support options. A few of the technical solutions within the customer support area are: • The Knowledge Base, which is a searchable database containing thousands of articles on topics ranging from schematic design entry and VHDL-based PLD design to PCB layout methodologies.
Chapter 20 Before you begin
Getting Started 1 Overview This chapter describes Schematics: what it is, what it can do, and how you can use it. This chapter has the following sections: Using Schematics on page 1-2 provides a broad overview and describes various functions. Example—Drawing a Schematic on page 1-4 provides a step-by-step example of creating a schematic.
Chapter 1 Getting Started Using Schematics Schematics is a schematic capture front-end program that provides a convenient system for: • creating and managing circuit drawings. • setting up and running simulations. • evaluating simulation results using MicroSim Probe. • creating netlists for external PCB layout packages. An important prerequisite to building a schematic is availability of proper symbols for assembly.
Using Schematics packages PCB Layout footprints package definitions layout netlist file symbols symbol definitions PSpice Schematics models layout ECO file netlist & packaging information back annotation Probe Probe markers circuit file netlist & simulation directives Figure 1 Interaction of Sim Software component description file Bill of Materials Programs and reports Files Probe data file PSpice A/D simulation results simulation audit simulation output file 3
Chapter 1 Getting Started Example—Drawing a Schematic The following example demonstrates the basic drawing features for drawing a schematic. It shows you how to: • start the schematic editor and begin a new design. • find out which libraries are configured for Schematics. • place parts on a schematic. • connect the part using wires and buses. • label wires and buses. • change reference designators and part values. • move parts, wires and text. • use ports on a schematic.
Example—Drawing a Schematic Figure 2 Opto-isolated, Addressable Serial-to-parallel Converter Circuit 5
Chapter 1 Getting Started Starting a New Design Start the schematic editor by double-clicking on the Schematics icon in the Orcad program group. An empty schematic page displays. If you already have Schematics running with another schematic displayed, click the New File icon to start a new schematic. Command Line Options PSpice Schematics supports a number of command line options that enable you to customize the start-up mode.
Example—Drawing a Schematic Checking Symbol Libraries Configuration When you installed Schematics, you selected a set of libraries to be installed. These are global libraries, which means the symbols contained in them are available to be used in any new or existing schematic. Check to see that you have the correct symbol libraries configured for this example: 1 From the Options menu, select Editor Configuration. 2 Check that the following libraries are included in the Libraries list box: 7400 [.slb,.
Chapter 1 Getting Started Selecting and Placing Parts 1 From the Draw menu, select Get New Part to display the Part Browser dialog box. 2 There are several ways to select a part in the Part Browser dialog box: One of two Part Browser dialog boxes may appear: the Part Browser Advanced or the Part Browser Basic. If in the Part Browser Advanced dialog appears, click <
Example—Drawing a Schematic Placing resistors R1 and R2 1 From the Draw menu, select Get New Part to display the Part Browser dialog box (shown on 1-8). 2 Type R in the Part Name text box. 3 Click Place & Close. The outline of the resistor becomes attached to the pointer. Note that as you move the pointer, the X and Y coordinates at the left of the Status Bar (bottom of the window) change. These coordinates show the location of the pointer from origin 0,0 (upper left corner) to the closest 0.
Chapter 1 Getting Started 3 Place the pointer in the approximate position for the placement of R3 and click to place the part. 4 Press M three times to place three more resistors above the first. Placing resistors R7 through R10 Table 1 Remaining Parts to be Placed 1 From the Get Recent Part list box on the toolbar, select R. 2 Press C+R to rotate the resistor before placing it. Reference Designator Part Name 3 Place four resistors in the approximate locations of R7, R8, R9, and R10.
Example—Drawing a Schematic Drawing and Labeling Wires Draw the wire labeled dataclk to connect pin 8 (CLK) on U3 and pin 1 (A) on U8A. Drawing the dataclk wire 1 Click the Draw Wire button. The pencil pointer indicates that you are ready to draw a wire. 2 Click pin 8 of U3 to begin the wire. 3 Following the illustration in Figure 2, click where you want each vertex of the wire. Each click ends a wire segment and starts a new one.
Chapter 1 Getting Started Buses must be labeled. Examples of legal bus names are: Drawing and Labeling Buses DB[0-12] DB[0:12] DB[0..12] DB0, DB1, CLK Draw the bus labeled DB[1-12]. Drawing the bus 1 Click the Draw Bus button. The pointer is now shaped like a pencil (as it was when you were drawing wires). 2 Click where you want to start the bus. 3 Click the pointer where you want to end the bus. 4 Right-click to stop drawing buses.
Example—Drawing a Schematic Labeling the wires connected to the bus You can use Auto-Naming to label a uniform collection of wires. 1 Note Each wire connecting to a bus must be labeled with the name of one of the signals on the bus. From the Options menu, select Auto-Naming to display the Auto Naming dialog box. a In the Wire/Port Labels frame, select the Enable Auto-Increment check box. b In the Label Template text box, type DB1, which is the label for the first wire in the series.
Chapter 1 Getting Started Changing Reference Designators and Part Values Change part values and reference designators by double-clicking them and typing a new value in the dialog box. Changing U8A to U9B When you place a part on the schematic, the part is automatically assigned a reference designator and a gate (if it is a multi-part component). For instance, when you placed the 74123 part, it was assigned something like U8A (that is, reference designator U8 and gate A).
Example—Drawing a Schematic Moving Parts, Wires, and Text Move parts, wires, buses, and text by clicking to select them, and dragging them to a new location. To maintain connectivity when moving parts, wires, or buses, enable the rubberbanding option. For information on how to enable the rubberbanding option, see Rubberbanding on page 4-111. Moving resistor R1 up one grid 1 Click the resistor to select it. 2 Drag the resistor up one grid. 3 Place the resistor at the new location.
Chapter 1 Getting Started Placing Ports Ports in Schematics identify signals that are inputs or outputs to a schematic. Place ports in the same way that you place other parts. Placing the port 16 1 From the Draw menu, select Get New Part to display the Part Browser dialog box (shown on page 8). 2 Click Libraries to display the Library Browser dialog box. 3 In the Library list box, select port.slb. 4 In the Part list box, select GLOBAL (which is the name of a global port symbol). 5 Click OK.
Example—Drawing a Schematic Labeling the port 1 Double-click the port symbol to display the Set Attribute Value dialog box. 2 Type DAT in the LABEL text box. 3 Click OK. Now place two more ports and label them CLK and RTN as shown in Figure 2. Placing Power and Ground Symbols Power and ground symbols are types of global port symbols in Schematics. The label on the port defines the name of the power supply. Placing +5-volt power supplies 1 Type +5V in the Get Recent Part list box on the toolbar.
Chapter 1 Getting Started Placing ground symbols 1 In the Get Recent Part list box on the toolbar, type EGND. 2 Press R to select the part. 3 Move the pointer to the location of the ground symbol and click to place the symbol. 4 Move the pointer and click to place the other four ground symbols. 5 Right-click to stop placing parts. Saving Your Work Click the File Save button, or select Save (or Save As) from the File menu to save the schematic.
Using Design Manager 2 Overview This chapter provides introductory information about the Design Manager. This chapter has the following sections: Understanding Design Manager on page 2-20 describes the purpose and uses for Design Manager. Managing Your Files in the Workspace on page 2-22 explains what a workspace is and how to manage your files within it. Design Manager Functions on page 2-23 describes Design Manager functions and activities.
Chapter 2 Using Design Manager Understanding Design Manager Design Manager allows you to browse, manage, archive, and restore your design files.
Understanding Design Manager 21
Chapter 2 Using Design Manager Managing Your Files in the Workspace Multiple workspaces, in their own windows, can be open simultaneously for browsing and file management activities. Design Manager views a file’s top-level folder (as seen in Windows Explorer) as a workspace and assigns it the name of the top-level folder. Although workspaces are actual folders, categories are not.
Design Manager Functions Design Manager Functions The following describes Design Manager functions and activities: General characteristics • availability for use without other Orcad programs running • automatic categorization of design-related files, sorted into file-type categories, within a workspace • ability to have multiple workspaces, in their own windows, open simultaneously • two methods (view by Category and view by Name) with which you can view and manage all files within a selected works
Chapter 2 Using Design Manager Archive and restore • 24 archive and restore to save a design and all of its references, package files for shipment to another location, save disk space, and localize externally referenced and shared files into a selected workspace
Starting the Design Manager Starting the Design Manager The Design Manager is automatically opened and minimized when you open PSpice Schematics. You can also open Design Manager to view and manage files without first opening Schematics. Opening the Design Manager outside of Schematics 1 On the task bar, click the Start button. 2 Point to Programs. 3 Point to the Orcad folder. 4 Click Orcad Design Manager. Design Manager opens with the Category view in effect.
Chapter 2 Using Design Manager 26
Using the Schematic Editor 3 Overview This chapter provides background information about the schematic editor. To see specific step-by-step instructions for creating a design, see Chapter 4, Creating and Editing Designs. This chapter has the following sections: Components of a Design on page 3-29 introduces and explains the components of a design. Main Window on page 3-32 describes the user interface to the schematic editor.
Chapter 3 Using the Schematic Editor of your schematic, in addition to specifying colors and sizes. Zooming and Panning in Schematics on page 3-68 tells how to zoom in and out of the drawing, refresh the screen display, pan to various sections of the drawing and fit the drawing to the page. Using the Message Viewer on page 3-73 describes the Message Viewer that displays system messages and explains the various displays and controls.
Components of a Design Components of a Design A schematic consists of: • symbols • attributes • wires • buses • text items Schematics can have either a flat or hierarchical structure, depending on the way you decide to implement your design. PSpice Schematics uses two basic types of parts: primitive and hierarchical.
Chapter 3 Using the Schematic Editor Symbols Symbols are the graphical representation of parts, ports, and other schematic elements. They are grouped by functionality into symbol libraries. Each symbol contains a specific set of attributes that define the symbol. You can edit these attributes as well as create new attributes. Symbols can share similar attributes and graphics. Hierarchical symbols represent schematics and are the mechanism that you use to create hierarchical designs.
Components of a Design Connections Parts and ports contain one or more pins where connections are made. Electrical connections are formed by wire and bus segments joining pins and other wire and bus segments. Connections are also formed by attaching pins directly to pins. PSpice Schematics represents each such electrical connection by a junction. Junctions are made visible when three or more connected items converge at the junction. Junctions are created and removed automatically.
Chapter 3 Using the Schematic Editor Main Window When you start PSpice Schematics, a schematic editor window opens and displays a single schematic page. You have the option of opening additional schematic editor windows. Use these windows to: • display different schematics. • display different portions of a single schematic page. • display different pages of the same schematic. • display different levels of hierarchy from the same schematic. • display a separate symbol editor window.
Main Window Toolbars Toolbar buttons provide shortcuts for performing common actions. All toolbars are dockable, so they may be moved to any location on the schematic. Standard Schematics The Standard Schematics toolbar provides shortcuts to standard Windows commands. Table 2 To “dock” toolbars: 1 Click anywhere on the toolbar (except on the buttons). 2 Drag it to the desired location in the schematic window or on your desktop.
Chapter 3 Using the Schematic Editor Table 2 Standard Schematics Toolbar Button Name Function Page Redraw refreshes the active schematic 3-41 page screen display Zoom In views a smaller area of schematic 3-68 Zoom Out views a larger area of schematic 3-69 Zoom Area views a selected area of schematic 3-68 Zoom to Fit Page fits the view to show all items 3-70 on the page 34
Main Window Drawing The Drawing toolbar provides shortcuts for drawing and editing items on your schematic.
Chapter 3 Using the Schematic Editor Simulation The Simulation toolbar provides shortcuts for setting up analyses, running a simulation, and viewing results. Refer to the Viewing Results on the Schematic chapter of your PSpice A/D User’s Guide for further information on simulation in Schematics.
Main Window Table 4 Button Simulation Toolbar Name Function Page Enable Bias Voltage Display toggles the display of bias voltage * Show/Hide Voltage on Selected Net(s) toggles the display of voltages for selected wires * Enable Bias Current Display toggles the display of bias current * Show/Hide Currents on Selected Part(s) toggles the display of currents for selected device pins * * Refer to the Viewing Results on the Schematic chapter in your PSpice user’s guide for information about how
Chapter 3 Using the Schematic Editor Annotation Graphics The Annotation Graphics toolbar provides shortcuts for drawing or inserting non-electrical information onto your schematic.
Main Window Status Bar The status bar is located at the bottom of the schematic editor window and provides the following: • X and Y coordinates of the pointer. Use the Display Options selection under the Options menu to toggle display of X and Y coordinates. • A message area that provides: • a brief description of the function that will be performed if you click the toolbar button at the present pointer location. • a brief description of the function to be performed.
Chapter 3 Using the Schematic Editor Table 6 Schematic Editor Function Keys Function keys 4 through 9 are toggle keys. Pressing the key enables the feature, and pressing S plus the key disables the feature.
Configuring PSpice Schematics Configuring PSpice Schematics The following list summarizes the different types of options you can configure in PSpice Schematics. Customizing configurable options allows you to use PSpice Schematics in the way that best suits your needs and requirements.
Chapter 3 Using the Schematic Editor Configuring Symbol Libraries There are two major elements that work together in Schematics that let you place symbols into your design: • symbol libraries • library search list Symbol libraries are located in library directories. The library search list is in the Part Browser and the Editor Configuration dialog box under the Options menu. A library name must be in the library search list to be available for placing its symbols.
Configuring PSpice Schematics Types of Libraries Schematics recognizes two types of libraries: This library... Is available... global to all schematic designs. They are listed in the pspice.ini file and are automatically loaded into the library search list for every design. Global libraries appear in the library search list with an asterisk (*) preceding the library name. local to designs within which they are saved. Schematics always places local library names at the top of the library search list.
Chapter 3 Using the Schematic Editor User-Defined Symbol Libraries You can create global and local symbol libraries, and add them to the default directory or to another directory of your choice. Once created, you can perform all the same actions as listed in Default Library Directory on page 3-43. Note When adding a symbol library to the library search list, placement in the list is important. If more than one library contains the same symbol name, Schematics uses only the first one it encounters.
Configuring PSpice Schematics 3 In the list of libraries, select the location for the new library. A new global library will be added directly above the library you select. A new local library will be placed above the first global library name in the list. 4 If the library you are adding is a symbol library, select the Symbol check box. If the library you are adding has an associated package library, select the Package check box. 5 In the Library Name text box, type the name of the library.
Chapter 3 Using the Schematic Editor Removing Library Names When removing a library name, it is only removed from the configured libraries list. The library is not deleted. If you no longer need a library name in the list of configured libraries, you can remove it from the list of configured libraries. Removing a library name Options Menu 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box (shown on 3-44).
Configuring PSpice Schematics Do not type a file name extension; the file name extension is appended automatically. 5 Click Change. 6 Click OK to exit the Library Setting dialog box. 7 In the Editor Configuration dialog box, click OK. Changing the Search Order The way that PSpice Schematics searches libraries for a symbol follows the order in which the libraries are configured in the list. You can change the position of a library in the list.
Chapter 3 Using the Schematic Editor The repositioned library name is inserted above the selected name. 9 Click OK to exit the Library Setting dialog box. 10 In the Editor Configuration dialog box, click OK. Changing the Search Path Note Local libraries are first looked for in the directory where the schematic resides. PSpice Schematics looks for a library according to the path(s) specified by the Library Path in the Editor Configuration dialog box.
Configuring PSpice Schematics Changing Page Size PSpice Schematics supports standard page sizes A through E and A0 through A4. It also allows you to specify a user defined page size. Changing the page size 1 From the Options menu, click Page Size to display the Page Size dialog box. 2 Click the appropriate button to select a pre-defined page size, or indicate a User Defined Size by typing the page dimensions in the Horiz: and Vert: text boxes.
Chapter 3 Using the Schematic Editor Changing Page Settings Note If you are using zoned borders, make sure the Display check box for the Page Boundary layer in the Display Preferences dialog box is enabled (see Controlling the Display in PSpice Schematics on page 3-60). For all page sizes, you can change the border style, the drawing area, and the pin-to-pin spacing. Border Style Schematics provides two border styles: zoned and outline. Figure 3 illustrates the two styles.
Configuring PSpice Schematics Table 7 Zoned Border Default Decimal Parameters Type Dimension* Vertical Horizontal Zones Margin Zones Margin A 8.5 x 11 2 .25 2 .38 B 11 x 17 2 .62 4 .38 C 17 x 22 4 .5 4 .75 D 22 x 34 4 1.0 8 .5 E 34 x 44 8 .5 8 1.0 * in inches The following table lists the default metric page sizes and their configurations.
Chapter 3 Using the Schematic Editor Changing the border style You can specify which border style to use through the Editor Configuration dialog box. The current drawing and all subsequent new drawings use the style you select. Options Menu 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box. 2 Click Page Settings to display the Page Settings dialog box. 3 Select the page size for which you want to set the border style.
Configuring PSpice Schematics 4 Select the Outline or Zoned border style. For style... Do this... Outline 1 In the Borders frame, click the Outline button. 2 Click OK to accept the Outline border and exit the Page Settings dialog box. 1 In the Borders frame, click the Zoned button. 2 Type the number of zones for each axis. 3 Type the margin sizes for each axis. 4 Select letters or numbers for zone designators in each plane.
Chapter 3 Using the Schematic Editor Drawing Area Changing the drawing area size Note Drawing areas for zoned and outline border types are the same size, (see Figure 3 on page 3-50). 54 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box (shown on 3-52). 2 Click Page Settings to display the Page Settings dialog box. 3 In the Width and Height text boxes, type the drawing area dimensions for the page size.
Configuring PSpice Schematics Pin-to-Pin Spacing You can scale symbols so they will appear larger or smaller on the schematic. You do this by changing the pin-to-pin spacing for a given page size. Changing the pin-to-pin spacing 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box (shown on 3-52). 2 Click Page Settings to display the Page Settings dialog box (shown on 3-54). 3 In the Pin-to-Pin Spacing text box, type a new value. 4 Click OK.
Chapter 3 Using the Schematic Editor Stay-on-Grid Stay-on-grid controls the method of object placement. When Stay-on-Grid is enabled, the objects are forced onto grid when placed. We recommend that you enable this so that electrical connections are made correctly. Enabling or disabling stay-on-grid 1 From the Options menu, select Display Options. 2 Select or clear the Stay-on-Grid check box to enable or disable Stay-on-Grid. 3 Click OK.
Configuring PSpice Schematics Snap-to-Pin Snap-to-pin, when enabled, causes the endpoint of a wire or bus segment to snap to the nearest pin if one is found inside the radius defined by the Gravity setting. Enabling or disabling snap-to-pin 1 From the Options menu, select Display Options. 2 Select or clear the Snap-to-Pin check box to enable or disable snap-to-pin. 3 Click OK. Grid Spacing Grid Spacing defines the horizontal and vertical grid spacing on your drawing area.
Chapter 3 Using the Schematic Editor Text Grid Text Grid allows you to set the grid spacing for text separately from the drawing grid spacing. The text grid is usually set to some smaller percentage of the drawing grid. This allows you to align text between drawing grid points. Enabling text grid and specifying text grid size 1 From the Options menu, select Display Options. 2 In the Text Grid frame, select the Stay-on-Grid check box to enable the text grid.
Configuring PSpice Schematics When Autosave is enabled, PSpice Schematics creates a temporary file with the same name as the active working file, and a file name extension ending in ‘v’ (for example, “.scv,” “.slv,” “.plv”). If you have a power outage or system failure, you can retrieve your work from these files. The temporary files are deleted each time a schematic or library is successfully closed or saved.
Chapter 3 Using the Schematic Editor Controlling the Display in PSpice Schematics PSpice Schematics allows you to define what elements of a design you want to display and print. This means you can set different display properties for each element of your schematic. In the Display Preferences dialog box, the default colors, styles, fonts, and sizes of each display layer are established.
Controlling the Display in PSpice Schematics Displaying or printing default properties 1 From the Options menu, select Display Preferences to display the Display Preferences dialog box. Options Menu 2 From the Display Layers list, select the appropriate display layer (or layers). To select more than one layer consecutively: 3 Click the General tab. 1 Hold down S. 4 Select or clear the Display check box to enable or disable display of the selected layers.
Chapter 3 Using the Schematic Editor Changing Fonts If you are rotating text objects, use TrueType fonts to prevent the display from becoming distorted. To change the default fonts PSpice Schematics uses to display and print text, use the Display Preferences dialog box. Selecting a font Options Menu 62 1 From the Options menu, select Display Preferences to display the Display Preferences dialog box. 2 Select one or more layers from the Display Layers list. 3 Click the Text tab.
Controlling the Display in PSpice Schematics 5 Select a font and size from their corresponding list boxes and click OK. A sample of the selected font is shown in the Sample box. 6 Enter a size in either inches or millimeters, or accept the system default for the selected font. 7 Select a color from the Color list box. 8 Click Apply to apply the changes and keep the dialog box displayed for further changes, or click OK to apply the changes and close the dialog box.
Chapter 3 Using the Schematic Editor Changing Application Settings You have the option to change the location of the .exe files of the programs that Schematics interfaces with. You can also configure a different text editor (besides WordPad) and specify an initialization file other than the installed default initialization file. Changing where to find programs 64 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box.
Controlling the Display in PSpice Schematics The Simulate Command frame shows the path that PSpice Schematics uses to run MicroSim PSpice A/D. 3 To change the path name, type a new path name in the Command text box. 4 Similarly, to change any of the other command lines, click to select the command in the Other Commands list box and type a new path name in the Command text box. 5 Click OK to exit the App Settings dialog box. 6 In the Editor Configuration dialog box, click OK.
Chapter 3 Using the Schematic Editor 4 Type the file name of the configuration file in the text box. 5 Click OK to exit the App Setting dialog box. 6 In the Editor Configuration dialog box, click OK. Specifying a different text editor Editing text in PSpice Schematics is done through the WordPad program. You have the option to specify a different text editor. 66 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box (shown on 3-65).
Controlling the Display in PSpice Schematics Changing the Get Recent Part List Size The Get Recent Part list box on the toolbar contains a scroll-down list of recently placed parts. The default length of this list is ten items. To change the length of the list, use a text editor to edit the MRPLISTSIZE item in the [SCHEMATICS] section of the pspice.ini file.
Chapter 3 Using the Schematic Editor Zooming and Panning in Schematics Zooming When working on a design, you can zoom in (enlarge the view) or zoom out (reduce the view) to view a larger or smaller portion of the schematic window. Zooming in reduces the area viewed and enlarges the objects viewed. Zooming out increases the area viewed and reduces the size of the objects viewed. Zooming in 1 From the View menu, select In. 2 Move the pointer to the desired center of the zoom action and click.
Zooming and Panning in Schematics Zooming out about the center of the window 1 Click the Zoom Out button. or press C+O The amount of reduction is determined by the Zoom Scale Factor (see Setting Zoom Parameters on page 3-69). Zooming out to view the full schematic page 1 From the View menu, select Entire Page.
Chapter 3 Using the Schematic Editor This value defines the percentage of the work space to be filled with the complete schematic when you select View Fit. Type a decimal value between 50 and 100. A typical value is 90. 4 Click OK. Fitting to a Page All of the parts, wires and text within the active window (excluding the title block) are displayed by fitting the view to the page. Fitting the view to the page 1 or press C+N Click the Zoom to Fit Page button, or select Fit from the View menu.
Zooming and Panning in Schematics Automatic Panning If Auto Pan is enabled, the pointer turns to a solid black arrow when you move it to the edge of the window. If you leave the arrow at the edge of the window for a few moments, the view pans in the direction of the arrow. You can pan up, down, left, and right using this method. Enabling Automatic Panning 1 From the Options menu, select Pan & Zoom to display the Pan & Zoom dialog box. Options Menu 2 In the Auto Pan frame, select the Enable check box.
Chapter 3 Using the Schematic Editor Setting Auto Pan sensitivity The Auto Pan sensitivity setting determines how long the pointer must remain on the window border before the panning takes place. 1 From the Options menu, click Pan & Zoom to display the Pan & Zoom dialog box (shown on page 3-71). 2 In the Auto Pan frame, type a value in the Sensitivity text box. The value in the text box is the time delay in milliseconds. The default is 1000 milliseconds. 3 Click OK.
Using the Message Viewer Using the Message Viewer The Message Viewer displays text describing a condition, status or other information concerning the operation of PSpice Schematics. The Message Viewer appears when any condition generates a message that requires you to be informed. For example, warnings and error messages that occur during netlisting will appear in the Message Viewer. The Message Viewer uses all standard Windows controls for scrolling, sizing, and selecting.
Chapter 3 Using the Schematic Editor Online Help Another way to view online Help is: 1 Right-click in the message area to display a menu. The Message Viewer has an online Help feature that allows you to view a help message directly relating to the currently selected message. To view a context-sensitive Help message: 2 Click Help On to view a context-sensitive Help message. 1 In the message viewer window, select the message. 2 Press 1.
Using the Message Viewer Table 1: Color Indication Blue Informational message. No user action is required. Yellow Warning message. May require some user action. Red Error message. Must be corrected before continuing. Black Fatal error message. Indicates a non-recoverable error condition.
Chapter 3 Using the Schematic Editor Additional Information Some messages contain additional text. That is, the message contains several lines of information while only one line displays. Lines containing additional information are indicated by a plus sign in the severity marker preceding the message text. When the Message Viewer contains any messages with additional information, the More Info button on the tool bar is active.
Creating and Editing Designs 4 Overview This chapter contains the step-by-step procedures for creating, editing, and printing a schematic, which includes: Starting the Schematic Editor on page 4-79 describes how to start the schematic editor and how to open a new or existing file. Finding Parts on page 4-80 describes how to find parts by name or description, and by searching the symbol libraries.
Chapter 4 Creating and Editing Designs Using Wires and Buses on page 4-104 describes drawing and labeling wires and buses, in addition to describing the drawing options that affect the placement of wires and buses. Using Ports on page 4-114 describes the use of off-page and global ports. Selecting and Moving Objects and Attributes on page 4-116 describes how to select and move parts, wires, and attributes.
Starting the Schematic Editor Starting the Schematic Editor Start the schematic editor by double-clicking on the Schematics icon in the Orcad program group. An empty schematic page appears. If you already have Schematics running with another schematic open, click the New File button to start a new schematic. Opening a File To open a new file, click the New File button. An empty schematic page appears. To open an existing file and display the schematic for editing, click the Open File button.
Chapter 4 Creating and Editing Designs Finding Parts Simulation Checklist When you are drawing a design for simulation, keep the following in mind: • The symbols that you place must have corresponding simulation models associated with them. • The design will need sources of stimulus. • For any part that has an associated simulation model, unmodeled pins are indicated by a broken pin.
Finding Parts Getting Parts by Name The Get Recent Part list box on the toolbar provides a list of the most recently used parts. You can also type a name in the Get Recent Part list box to select a part. Selecting a part by name 1 In the Get Recent Part list box, type the name of the part you want to place. 2 Press R. 3 Move the outline of the selected symbol to any location on the schematic and click to place the part. 4 Right-click to stop placing parts.
Chapter 4 Creating and Editing Designs Searching for Parts in the Libraries Symbol libraries contain symbols for many parts. There are three methods for selecting parts from libraries: • Search for the part by name. • Search for the part by description. • Browse through the symbol libraries. Each of these methods are described below. Selecting a part by name 1 From the Draw menu, select Get New Part to display one of the Part Browser dialog boxes.
Finding Parts 4 Move the outline of the selected symbol to any location on the schematic and click to place the part. 5 Right-click to stop placing parts. Selecting a part by description 1 Click the Get New Part button to display the Part Browser dialog box (see 4-82). Note You may display one of two Part Browser dialog boxes: the Part Browser Advanced or the Part Browser Basic. If the Part Browser Basic dialog box appears, click Advanced to display the Part Browser Advanced dialog box.
Chapter 4 Creating and Editing Designs 7 Move the outline of the selected symbol to any location on the schematic and click to place the part. 8 Right-click to stop placing parts. Browsing symbol libraries to select a part 1 Note 2 Click the Get New Part button to display the Part Browser dialog box (see 4-82). One of two Part Browser dialog boxes may appear: the Part Browser Advanced and the Part Browser Basic.
Placing and Editing Parts Placing and Editing Parts After you have selected a part, you can place one or more instances of the part on the schematic. When the part is selected, an outline of the selected part appears attached to the pointer. Placing a symbol on the schematic 1 Click the Get New Part button to select the part from a symbol library. 2 Move the symbol outline to the location you want to place the symbol and click.
Chapter 4 Creating and Editing Designs Rotating and Flipping Parts In PSpice Schematics, you can rotate and flip (mirror) parts or entire areas of a schematic. A rotated part is rotated 90° counter-clockwise. A flipped part is mirrored about the Y axis. Rotating and flipping can occur during one of the following: Rotating a Part R1 • while dragging (before placement) • after placement Rotating Parts Rotating a part before placing it 1 Select a part to be placed.
Placing and Editing Parts Flipping Parts Flipping a part before placing it 1 Select the part to be placed. 2 Press C+F to flip it. The symbol outline is a mirror image of the original image. Each time you press C+F, the image will flip about the vertical axis. Flipping a Part M1 VN0120N2 Default Flipping an already placed part 1 Select the part. 2 Press C+F to flip it. Flipping an area of the schematic 1 Drag the mouse to select and outline the area to be flipped.
Chapter 4 Creating and Editing Designs Editing Part Attributes Parts, ports, wires (nets), buses and most other symbols have associated attributes. An attribute consists of a name and an associated value. (See Attributes on page 3-30.) You can create new attributes or edit existing attributes of a part on the schematic. These functions are performed in the Attribute Editing dialog box. Editing Attributes Editing an attribute 1 Double-click the part to display the Attribute Editing dialog box.
Placing and Editing Parts The letter a indicates that the attribute has been annotated as a result of back annotation or has been assigned by the packager. Any changes you make to the part attributes are made to the individual part instance you selected. The original part contained in the symbol library remains unchanged. Attribute names can contain any alphanumeric characters (A–Z, 0–9) and the underscore character. Attributes cannot be self-referencing.
Chapter 4 Creating and Editing Designs Adding Attributes Adding a new attribute 1 Double-click the part to display the Attribute Editing dialog box (see 4-88). 2 Double-click in the Name text box and type the new attribute name. 3 Press F and type the new attribute value in the Value text box. 4 Click Save Attr. 5 Click OK. The new attribute and its value apply only to the part instance you are editing on the current schematic.
Placing and Editing Parts 3 Click Change Display to display the Change Attribute dialog box. 4 Select one of the option buttons in the What to Display frame. Your choices are: With many attributes such as the package reference and reference designator, only the value displays. With others, such as package type, neither the name nor the value displays. • Display the name of the attribute only. 5 Click OK to close the Change Attribute dialog box. 6 In the Attribute Editing dialog box, click OK.
Chapter 4 Creating and Editing Designs 4 Select or type a value for any of the Display Characteristics. You can change any of the characteristics as described in Table 9. 5 Click OK to close the Change Attribute dialog box. 6 Click OK to close the Attribute Editing dialog box. This procedure only changes the display characteristics for the attributes of the one instance of this part on the current schematic.
Placing and Editing Parts Global Editing of Attributes PSpice Schematics allows you to change an attribute on multiple parts at the same time. Assigning the same attribute value to multiple parts 1 Select more than one part, or select an area of the drawing enclosing the parts. 2 Select the Edit Attributes button. A confirmation dialog box appears asking if you want to globally edit attributes of all selected items. 3 Click Yes to display the Global Edit Attributes dialog box.
Chapter 4 Creating and Editing Designs Editing the Default Attributes of a Symbol When placing parts, you might want to change the value of an attribute for all parts of a certain type, such as a resistor. For example, you might want to change the default value for all resistors being placed from a value of 1 Kohm to 10 Kohm. Changing the default value of a resistor 1 Select a resistor symbol on the schematic. 2 Click the Edit Symbol button to display the resistor symbol in the symbol editor window.
Placing and Editing Parts 11 Type a name in the File Name text box. 12 Click Save. You are prompted to add the library to the list of configured libraries. 13 Click Yes. Repeating Part Placements If you are placing parts in line with each other and evenly spaced, use the Auto-Repeat function. Automatically repeating part placements Before selecting the part for placement, enable the Auto-Repeat function and set the offset spacing.
Chapter 4 Creating and Editing Designs Horiz. Offset 00.00 Vertical Offset 00.30 Horiz. Offset 00.00 Vertical Offset 00.50 Horiz. Offset 00.30 Vertical Offset 00.00 Horiz. Offset 00.50 Vertical Offset 00.100 Figure 4 Placing Resistors with Various Vertical and Horizontal Offsets Note Use 8 and S8 to enable and disable Auto-Repeat, respectively. If you do not need to change the offsets, this is a convenient way to quickly place arrays of parts and wires. 4 Select the part from the symbol library.
Placing and Editing Parts • Right-click to stop placing the part without placing an additional part. The outline changes back to a pointer. Automatically Assigning Reference Designators The Auto Naming function is useful for assigning reference designators to parts as they are placed. The default starting reference designator number is 1. When placing resistors, the first one placed is R1, the second R2, and so on.
Chapter 4 Creating and Editing Designs Example—Using Auto-Repeat and Auto Naming Use the following procedure to create part of the drawing shown in Figure 5 using the Auto-Repeat and Auto Naming functions. Figure 5 Auto Naming for Bus Labels Placing the bus and part 98 1 Click the Draw Bus button. 2 Move the pencil-shaped pointer to the location of one end of the first bus segment. Click to start drawing the bus. 3 Click at each vertex of the bus. Double-click at the end of the bus.
Placing and Editing Parts Drawing the first wire segment connecting the part to the bus 1 Click the Draw Wire button. 2 Move the pencil-shaped pointer to a point on the bus where wire segment A[0] attaches to the bus. Click to start drawing the wire. 3 Move to pin D1 on U1 and double-click. Using Auto-Repeat to create the remaining wire segments 1 Enable Auto-Repeat (see Automatically repeating part placements on page 4-95). 2 Set the horizontal offset to 00.00 and the vertical offset to 00.10.
Chapter 4 Creating and Editing Designs Replacing Parts A single part on a schematic may be replaced easily. In addition, all parts of a given type on a page, or all pages of a multi-page design may be replaced. Instead of having to delete one part, find another in a library, and place the new part, you can replace the old with the new in one operation. Replacing a single part 1 Select the part to be replaced. 2 From the Edit menu, select Replace to display the Replace Part dialog box.
Placing and Editing Parts Replacing all parts of the same name 1 From the Edit menu, select Replace to display the Replace Part dialog box. 2 In the Target Part text box, type the name of the parts to be replaced. 3 In the Replacement text box, type the name of the replacement parts. 4 If you want the attribute values of the parts being replaced applied to the replacement parts, select the Keep Attribute Values check box.
Chapter 4 Creating and Editing Designs Placing Power and Ground Symbols Placing and editing power and ground symbols is the same as placing and editing other part symbols with the following considerations: In PSpice Schematics, power and ground symbols are a type of global port symbol. The label on the port defines the name of the power supply. • Power and ground symbols are contained in the “port.slb” symbol library. • You can use the symbol editor to create your own custom power and ground symbols.
Placing Power and Ground Symbols Creating Custom Power and Ground Symbols Because power and ground symbols are just like any other symbols, you can use the symbol editor to create your own custom power and ground symbols. See Drawing Symbol Graphics on page 6-178.
Chapter 4 Creating and Editing Designs Using Wires and Buses Parts and ports contain one or more pins to which connections can be made. Electrical connections are formed by joining pins of parts and ports with wires and buses. A junction dot appears where three items are joined. Drawing and Labeling Wires Drawing a wire 1 Click the Draw Wire button to change the pointer to a pencil shape. 2 Click to start the wire. 3 Click at each vertex of the wire.
Using Wires and Buses If a wire segment is added so its end-point intersects another wire segment (at a point other than its end-points), a junction is created and the original wire is split into two segments. All three segments become part of the same wire. You can place a label on selected wires, bus segments, or ports. Wire and bus segments may have multiple labels. Note A wire connected to a bus must be labeled with one of the signals on the bus.
Chapter 4 Creating and Editing Designs 2 Click the wire segment that you want to change. 3 Click to place a vertex. 4 Double-click to place the last vertex and stop rewiring. Drawing and Labeling Buses Note Buses must be labeled. The connectivity of buses and bus segments in PSpice Schematics is controlled by labeling. The rules of connectivity are: • A bus label specifies the signals it carries and the order of the signals.
Using Wires and Buses Drawing a bus 1 Click the Draw Bus button to change the pointer to a pencil shape. 2 Click to start the bus. 3 Click at each vertex of the bus. 4 Right-click to end the bus and change the pencil back to a pointer. Labeling a bus 1 Double-click the bus segment to display the Set Attribute Value dialog box (see 4-105). 2 Type the label in the LABEL text box. 3 Click OK.
Chapter 4 Creating and Editing Designs 2 Label the bus segment with a subset of the signals on the main bus. For example, you can label the bus segment DB[0:8] if the main bus is labeled DB[0:16]. Automatically Labeling Wires and Buses Use the Auto Naming function to set up the labeling of wires and ports. The syntax specified in the Label Template text box allows you to name a uniform collection of wires.
Using Wires and Buses Specifying Drawing Options Several options aid in drawing wires and buses and in placing parts. • The Orthogonal option constrains wires and buses to vertical and horizontal lines. • The Snap-to-Grid option keeps parts, wires, and buses aligned to grid lines. • The Snap-to-Pin option constrains wire and bus placements to the nearest pin. • The Rubberband option maintains connectivity between parts when they are moved.
Chapter 4 Creating and Editing Designs Enabling orthogonal drawing 1 From the Options menu, select Display Options. 2 In the Options frame, select or clear the Orthogonal check box to enable or disable orthogonality. 3 Click OK. Snap-to-Grid Stay-on-Grid must be enabled for Snap-to-Grid to be effective. Snap-to-grid controls the movement of the object while being moved for placement when Stay-on-Grid is enabled.
Using Wires and Buses Gravity Gravity specifies how close an object must be to a pin to snap to it. Gravity is only functional when snap-to-pin is enabled. Specifying gravity 1 From the Options menu, select Display Options (shown on page 4-110). 2 In the Snap-to-Pin frame, in the Gravity box, type the snap-to-pin gravity value. 3 Click OK. Gravity is only functional when snap-to-pin is enabled. Grid Spacing Grid Spacing defines the horizontal and vertical grid spacing on your drawing area.
Chapter 4 Creating and Editing Designs Figure 7 Rubberbanding with Orthogonal enabled Figure 8 Rubberbanding with Orthogonal disabled 112
Using Wires and Buses While you are moving an object (whether orthogonal is enabled or disabled), an X appears where a new connection will be made if the object is placed, and the pointer changes to a caution sign (see Figure 9 below). If you continue to move the object (away from the connection), the X disappears and the pointer returns to normal.
Chapter 4 Creating and Editing Designs Using Ports Signals can be connected without using wires or buses by connecting them to global or off-page ports and labeling the ports with the same name. A third type of port, interface port provides connections between the pins of a hierarchical block or symbol and the underlying schematic. Refer to Chapter 7, Creating and Editing Hierarchical Designs, the section on Using Interface Ports on page 7-236.
Using Ports Placing a global port 1 Click the Get New Part button to display a Part Browser dialog box, (see 4-82). 2 Click Libraries to display the Library Browser dialog box (see 3-45). 3 In the Library list, select port.slb. 4 In the Part list, double-click GLOBAL. 5 Click Place to place the global port, or click Place & Close to close the dialog box and place the global port. Note A quick way to place the global port is to type “global” in the Get Recent Part list box on the toolbar.
Chapter 4 Creating and Editing Designs Selecting and Moving Objects and Attributes Before performing any operation on a schematic object, you have to select the object. You can make multiple selections or select whole areas of the schematic. After you select an object, you can move, copy, delete, edit, cut, and paste that object. Selecting Selecting an object (a part, wire, or bus on the schematic) 1 Point to the object with the pointer and click to select it.
Selecting and Moving Objects and Attributes A rectangle is drawn around the attribute; a selection rectangle also appears around the object that the attribute belongs to. De-selecting selected objects 1 Click to select an object other than the selected object, or click in a blank area of the schematic. Moving Moving an object 1 Select an object (or group of objects). 2 Click the pointer on the object, or in the area designated by the selection rectangle.
Chapter 4 Creating and Editing Designs Finding a part When typing an attribute name and value, you can specify an exact value or use wildcards. 1 From the Edit menu, select Find to display the Find dialog box. 2 Specify the search criteria: An asterisk (*) is a wildcard that matches zero or more characters. For example, R* matches R, R1 and R12. A question mark (?) is a wildcard that matches any single character. For example, R? matches R1 but not R or R12.
Selecting and Moving Objects and Attributes Cutting, Copying, and Pasting PSpice Schematics provides several editing features that allow you to cut, copy, paste, copy to clipboard, delete, and undelete selected objects. All of these functions are available under the Edit menu. Most can be accessed from the keyboard. The cut, copy, copy to clipboard, and delete functions only apply when an object is selected.
Chapter 4 Creating and Editing Designs Pasting an object Shortcut: press C+V 1 From the Edit menu, select Paste to change the pointer to the shape of the object last cut or copied. 2 Click to place the object at the current pointer location. With Auto-Repeat enabled (see Repeating Part Placements on page 4-95), press M to place repeated copies of items from the buffer. Continue moving the pointer to various locations and clicking to place additional copies of the object. Right-click to stop pasting.
Selecting and Moving Objects and Attributes Copying to the Clipboard The Copy to Clipboard function copies objects within a selection rectangle to the Microsoft Windows Clipboard for use in other Windows programs. Electrical or connectivity information is not copied to the clipboard. This function is useful if you want to make a copy of your schematic to include in another type of file, such as a word processor file.
Chapter 4 Creating and Editing Designs Creating and Editing Title Blocks Each new schematic is created with a title block in the lower-right corner of the page. The title block is treated as an annotation symbol and each text field is an attribute. As such, you can edit the attributes of the title block much the same as you would the attributes of other objects. You can type information into the title block in the default format, or you can create a custom title block.
Creating and Editing Title Blocks Entering Information into the Title Block Entering information into the existing title block can be done in one of two ways: (1) by editing the attributes of the title block, in which case you can type information into any, or all fields of the title block, or (2) by editing an individual attribute of the title block.
Chapter 4 Creating and Editing Designs Editing one attribute of the title block 1 Double-click the attribute of the title block to display the Set Attribute Value dialog box. 2 Type or correct the information in the text box. 3 Click OK. Creating a Custom Title Block Because the title block is treated as a symbol, you can use the symbol editor to create your own custom title block or edit the existing title block to suit your requirements. See Chapter 6, Creating and Editing Symbols.
Creating and Editing Title Blocks Using a Custom Title Block Symbol After you have created a custom title block, you have to specify that block in order to use it in the current schematic. Specifying a new title block symbol 1 From the Options menu, select Editor Configuration to display the Editor Configuration dialog box (see 3-44). 2 In the Title Block Symbol text box, type the name of the title block symbol. 3 Click OK.
Chapter 4 Creating and Editing Designs Adding Non-Electrical Information Non-electrical information such as comments, tables, and graphics can be added to the schematic.
Adding Non-Electrical Information Resizing the text box 1 Select the text box to display its handles. 2 Click one of the handles and drag to resize the text box. To rotate the box, select it and press C+R. (See Rotating Parts on page 4-86.) Editing Text 1 Click inside the text box to modify or add text. Note The text will automatically wrap within the box as it is entered. Single Line Text Editing With the single line text option, you can continuously type text on one line.
Chapter 4 Creating and Editing Designs • Right-click to stop placing the text string without placing an additional one. The outline changes back to a pointer. Resizing the text box To rotate the box, select it and press C+R. (See Rotating Parts on page 4-86.) 1 Select the text to display the text box handles. 2 Click one of the handles and drag to resize the box to the size needed. Editing text Note The text will automatically wrap within the box as it is entered.
Adding Non-Electrical Information 3 Note 4 Select the appropriate properties for the text selected. In addition to changing the text properties, you can change the properties of the text box itself in the Frame area. Click OK. Setting the default text properties through Display Preferences 1 From the Options menu, select Display Preferences to display the Display Preferences dialog box. 2 Select one or more text layers from the Display Layers list (see 3-61 for how to select more than one layer).
Chapter 4 Creating and Editing Designs Note Changes made in the Display Preferences dialog box become the default settings for all schematics, but may be changed at any time. 3 Click the Text tab. 4 Select the appropriate properties. 5 Click Apply to apply the changes immediately and keep the dialog box open for further changes, or click OK to apply the changes and close the dialog box. Graphics Adding Graphics Graphics can be added directly onto your schematic.
Adding Non-Electrical Information Resizing annotation graphics 1 Select the object to display its handles. 2 Click one of the handles and drag to resize the object.
Chapter 4 Creating and Editing Designs Setting the default graphics properties through Display Preferences Note Changes made in the Display Preferences dialog box become the default settings for all schematics, but may be changed at any time. 132 1 From the Options menu, select Display Preferences to display the Display Preferences dialog box (shown on 4-129). 2 From the Display Layers list, select the Annotation Graphics layer. 3 Click the Graphics tab. 4 Select the appropriate properties.
Adding Non-Electrical Information Importing Bitmaps and Metafiles You can import bitmap (.bmp, .dib), Windows metafiles (.wmf), or enhanced metafiles (.emf) onto the schematic. Importing a graphic 1 From the Draw menu, select Insert Picture to display the Open dialog box. 2 Select the file type: Bitmaps or Metafiles. 3 Select a file from the window or type the path of the file location in the File Name text box. Note All imported graphics are imported by reference.
Chapter 4 Creating and Editing Designs Annotation Symbols Creating annotation symbols and adding them to a custom library allows you to easily use them in other designs. Creating annotation symbols 1 From the Edit menu, select Symbol to start the symbol editor. 2 From the File menu, select Open. Select the existing library where the annotation symbol will be saved. 3 4 Note 5 134 From the Part menu, select New to display the Definition dialog box.
Adding Non-Electrical Information 6 a Add any attributes to contain custom information for later use. b Click OK. From the File menu, select Save. Moving Non-Electrical Information Moving text, graphics, and annotation symbols 1 Select the object. 2 Place the pointer on the edge of the object and the annotation movement cursor becomes attached to the pointer. 3 Drag and place the object at the desired location on the page.
Chapter 4 Creating and Editing Designs Creating and Editing Multi-sheet Designs A schematic can contain one or more pages. As a schematic grows beyond a single page, ports are used to establish connectivity. Off-page ports provide connectivity between pages of the same schematic. Global ports provide connectivity across schematic pages to other global ports of the same name, anywhere in the schematic hierarchy. Off-page and global ports are named the same as the nets that they are connected to.
Creating and Editing Multi-sheet Designs Copying a page 1 From the Navigate menu, select Copy Page to display the Copy Page dialog box. 2 Select the schematic file from the Directory list. 3 Select a page number, if the page to be copied is part of a multi-page schematic. 4 Click OK to add the page to the current schematic after the current page and renumber all further pages. Navigate Menu Creating Connections Between Pages Use off-page ports to create connections between pages.
Chapter 4 Creating and Editing Designs Viewing Multiple Pages To view pages in a multi-page design, use the Previous Page, Next Page, and Select Page selections under the Navigate menu. Viewing the previous page 1 From the Navigate menu, select Previous Page. Viewing the next page 1 From the Navigate menu, select Next Page. Viewing a particular page 1 From the Navigate menu, select the Select Page option. 2 Double-click the desired page number and title. 3 Click OK.
Creating and Editing Multi-sheet Designs Deleting a Page To delete a page from a multi-page design, use Delete Page under the Navigate menu. Deleting a page 1 Navigate to the page you want to delete. 2 From the Navigate menu, select Delete Page to display a Delete Page confirmation dialog box. 3 Click OK to delete the page.
Chapter 4 Creating and Editing Designs Printing Your Design Printing options allow you to print one or more pages, or a selected area of a schematic. Printing the current page of the current schematic 1 Click the Print button. The page is immediately sent to the current (default) printer. Printing a selected area of the current page 1 Select an area of the schematic. (See Selecting on page 4-116.) 2 Click the Print button. The selected area is immediately sent to the current (default) printer.
Printing Your Design 3 Select one of the scaling options. See Scaling on page 4-141. 4 Select an Orientation of either Landscape or Portrait. Most schematics are in landscape format. Landscape is the schematic editor default format. 5 Click OK. Scaling Scaling options allow you to control the size of the printout. Auto-Fit Auto-fit scales the size of the page to print one schematic page per sheet of printer paper.
Chapter 4 Creating and Editing Designs In Landscape Mode A-size A-size EXAMPLE 1 B-size A-size Schematic Page Printed Paper In Portrait Mode B-size Schematic Page EXAMPLE 2 A-size Printed Paper Figure 13 Printing with Auto-Fit Enabled User-Definable Zoom Factor User-definable zoom factor allows you to set a custom zoom factor.
Printing Your Design With the zoom factor set to 200%, a B-size drawing will print on eight sheets of paper as shown in Figure 15. Doubling the zoom factor quadruples the number of printer pages needed to print a schematic.
Chapter 4 Creating and Editing Designs A-size 11 x 8 1/2 Schematic Page 8 1/2 x 11 8 1/2 x 11 Printed Paper B-size 17 x 11 Schematic Page 8 1/2 x 11 8 1/2 x 11 Printed Paper Figure 16 User-definable Zoom Enabled in Portrait Mode In landscape mode, using a 100% zoom factor, as shown in Figure 17: 144 • An A-size schematic will print on one sheet of A-size paper. • A B-size drawing will print on four sheets of A-size paper.
Printing Your Design A-size A-size 11x 8 1/2 11x 8 1/2 Schematic Page Printed Paper 11 x 8 1/2 11 x 8 1/2 B-size 17 x 11 Schematic Page 11 x 8 1/2 11 x 8 1/2 Printed Paper Figure 17 User-definable Zoom Enabled in Landscape Mode 145
Chapter 4 Creating and Editing Designs Closing the Schematic Editor File Menu You can close the schematic editor, thereby closing all open schematics. You can also close an open schematic without exiting the schematic editor. Closing the schematic editor To exit the schematic editor and close all currently open schematics, do one of the following: • From the File menu, select Exit. • In the upper-right corner of the schematic editor window, click the Close button.
Using the Symbol Editor 5 Overview The symbol editor enables you to do the following tasks: • create and edit symbols for use in the schematic editor • edit existing libraries • create new libraries This chapter provides background information about the symbol editor, which includes: Starting the Symbol Editor on page 5-151 describes procedures for starting and closing the symbol editor.
Chapter 5 Using the Symbol Editor Changing Text Characteristics on page 5-158 describes procedures for changing the text characteristics of attribute text, pin name and number display, and free-standing text. Changing Grid and Gravity on page 5-162 describes enabling and disabling grid, setting grid spacing, setting gravity and using text grid. Zooming and Panning on page 5-166 references the zoom and pan features of the symbol editor.
Components Components A component or device has several aspects associated with it: • symbol—the graphical representation used in drawing schematics • packaging information—defines the names of the package types (footprints) in which the component is available, the pin number assignments for those package types, and the number of gates (for multi-gate components) • footprint—used for board layout • simulation model—if the component can be simulated with PSpice A/D Symbols Symbols are created and mo
Chapter 5 Using the Symbol Editor Package definitions are created and modified with the PSpice Schematics symbol editor. Footprints The footprint for a component is the definition of its mechanical outline, pad pattern, identifiers, and physical extent (boundary). The package definition for a symbol defines the names of the footprints (package types) in which it is available. For each footprint, the package definition defines the physical pin number assignments for the pins.
Starting the Symbol Editor Starting the Symbol Editor Starting the symbol editor In the schematic editor, click the Edit Symbol button to create a new symbol editor document window if one does not already exist. If you already have a symbol editor window open, you will be prompted to save any unsaved changes to the active symbol. You can only have one symbol editor window open at a time. When you save the symbol library, any open schematics are updated with the changes made in the symbol editor.
Chapter 5 Using the Symbol Editor Saving your Changes To save newly created symbols or changes to existing symbols: 1 Click the File Save button on the toolbar. If the library is not configured for use in the schematic editor, you will be asked if you want to configure the library. Answer YES to make the symbols in the library available for use in PSpice Schematics. If the library is already configured, any schematics using symbols you have changed will be updated to use the new symbol.
Symbol Editor Window Symbol Editor Window When you start the symbol editor, the symbol editor window displays. Note You can only open one symbol editor window at a time and you can only edit one symbol at a time. Refreshing the Screen To clean up and refresh the screen, click the Redraw button on the toolbar. Menus There are a series of menus from which you can select the function you want to perform. The display and operation of the menus and submenus follow the standard Windows layout and operation.
Chapter 5 Using the Symbol Editor PSpice Schematics provides different menus for the schematic editor and for the symbol editor. The menus change as you change active windows. Toolbar Toolbar buttons provide shortcuts for performing common actions. To enable or disable the Toolbar display: View Menu 1 From the View menu, select Toolbar. A check mark next to the Toolbar menu item indicates that the toolbar is displayed.
Symbol Editor Window Table 10 Buttons Symbol Editor Toolbar Buttons Name Function Page Draw Circle draws a circle on the symbol 6-1 79 Draw Polyline draws a polyline or line on the symbol 6-1 79 Place Pins places pins on the symbol 6-1 80 Draw Text places a text string on the symbol 6-1 80 Insert Picture imports a bitmap (.bmp, .dib) or Windows metafiles (.wmf, .
Chapter 5 Using the Symbol Editor Title Bar The symbol editor window title bar displays the name of the symbol library and the symbol currently being edited. For example: [C:\ORCAD\LIB\PORT.SLB:GLOBAL] When you open a symbol editor window and have not specified a symbol for editing, the title bar displays: : This indicates you are editing a new symbol in a new library.
Symbol Editor Window Keyboard Table 11 lists the function keys you can use instead of menu selections to enable or disable certain functions. For those functions that toggle, pressing the function key enables the feature, and pressing S plus the function key disables the feature.
Chapter 5 Using the Symbol Editor Changing Text Characteristics For any text placed on your symbol, such as free standing text, pin names, attribute names, and values, there are options to set the desired text size, orientation, horizontal justification, and vertical justification. Attribute Text You can change the text characteristics of any attributes of the symbol. The text characteristic changes you make are only applied to the attribute that you are currently editing.
Changing Text Characteristics Table 12 Display Characteristics Characteristic Explanation Orient: Enables you to position the text horizontally, vertically, upside down, or down in relation to the defining point of the text string. Layer: Specifies a text display level as defined by the Set Display Level function under the Options menu. Defaults to Attribute Text Layer. You can specify a user defined layer. Size: Determines the size of the text of a displayed text item.
Chapter 5 Using the Symbol Editor Pin Name and Number Changing pin name text characteristics 1 Double-click the pin name or pin number to display the Change Pin dialog box. 2 Change any of the text characteristics as shown in Table 12. 3 Click OK. Changing pin number text characteristics 160 1 Double-click the pin name or pin number to display the Change Pin dialog box. 2 Click Edit Attributes to display the Attributes dialog box.
Changing Text Characteristics 3 Click to select an item in the list. Change any of the characteristics of the text in the Display Characteristics frame of the dialog box, as shown in Table 12. 4 Click OK. 5 In the Change Pin dialog box, click OK. Free-Standing Text You can change the text characteristics of any of the free-standing text that you have placed on the symbol. The changes you make are only applied to the text item you are currently editing.
Chapter 5 Using the Symbol Editor Changing Grid and Gravity The grid and gravity functions of PSpice Schematics eases your drawing tasks and can help make your schematic more precise. Grid On When Grid On is enabled, the grid is displayed in the drawing area of the schematic editor window. Enabling or disabling the grid display 1 Select Display Options from the Options menu to display the Display Options dialog box. 2 Select or clear the Grid On check box to enable or disable the grid display.
Changing Grid and Gravity Snap-to-Grid Snap-to-grid controls the movement of the object while being moved for placement. If Snap-to-Grid and Stay-on-Grid are both enabled, movement during object placement is in increments equal to the current grid spacing. If Snap-to-Grid or Stay-on-Grid is not selected, the object moves smoothly. The Stay-on-Grid command must be enabled for the Snap-to-Grid command to be effective. Enabling or disabling snap-to-grid 1 From the Options menu, select Display Options.
Chapter 5 Using the Symbol Editor Gravity The gravity setting determines how close the pointer must be to an object for the object to be selected when you click the pointer. The default is .03 inches (or .75mm). Specifying gravity Gravity is only functional when snap-to-pin is enabled. 164 1 From the Options menu, select Display Options. 2 In the Gravity text box, type the snap-to-pin gravity value. 3 Click OK.
Changing Grid and Gravity Text Grid Text Grid allows you to set the grid spacing for text separately from the normal grid spacing. The text grid is usually set to some smaller percentage of the regular drawing grid. This allows you to align text along smaller increments of the regular grid. Enabling text grid and specifying text grid size 1 From the Options menu, select Display Options. 2 Select the Text Stay-on-Grid check box to enable the text grid.
Chapter 5 Using the Symbol Editor Zooming and Panning The zoom and pan features in the symbol editor are the same as they are in the schematic editor. Refer to Zooming and Panning in Schematics on page 3-68.
Printing Symbols Printing Symbols Printing a symbol 1 From the File menu, select Print to display the Print dialog box. 2 To select the part or parts to be printed, do the following: a Select the Current Symbol Only check box to print the symbol being edited. b Select one or more parts from the Parts list. c Click Select All Parts to print all parts in the open library. 3 In the Content Options frame, select the check box to enable printing. The Content Options are described in Table 13.
Chapter 5 Using the Symbol Editor Table 13 168 Content Options Option Description Symbol Image specifies printing the graphics of the selected symbol Attributes specifies printing the attributes and the attribute values of the selected symbol Symbol Data specifies printing the description, type, Bbox dimensions, and origin position of the selected symbol Pin Data specifies printing the pin data of the selected symbol
Creating and Editing Symbols 6 Overview This chapter describes how to use the symbol editor to copy, create and edit symbols, which includes: Creating New Symbols on page 6-171 describes the four essential methods of creating a new symbol. Drawing Symbol Graphics on page 6-178 describes the assortment of drawing tools provided for creating and editing a symbol.
Chapter 6 Creating and Editing Symbols Configuring Custom Libraries on page 6-214 describes the procedure for making a custom library available in PSpice Schematics.
Creating New Symbols Creating New Symbols Following are the four methods for creating a new symbol: 1 Using the Symbol Wizard. • Use the wizard to create symbols from scratch. The wizard guides you through the steps for creating a symbol and also creates packaging information for the symbol. • Use the wizard to create symbols automatically for existing models. 2 Making a copy of an existing symbol under another name and modifying the copy.
Chapter 6 Creating and Editing Symbols When you start the Symbol Wizard you are taken through a progression of screens, which provide you with information, ask you questions, and present you with choices, based on your selection in the first screen (shown below). Starting the Symbol Wizard Note Symbol names cannot contain spaces. 172 1 From the Part menu, select Symbol Wizard. 2 Follow the instructions that appear on the screen.
Creating New Symbols Creating a Symbol by Copying Another Symbol An easy way to create a symbol is to make a copy of a similar symbol and modify the copy. Making a Copy of a Symbol Copying a symbol from another library 1 From the Part menu, select Copy to display the Copy Part dialog box. 2 Click Select Lib in the Open dialog box, and select a library. Part Menu PSpice Schematics lists all of the library parts in the Parts box.
Chapter 6 Creating and Editing Symbols Importing a symbol definition Import enables you to import a symbol that has been previously exported (see Exporting a symbol on page 6-174) and incorporate it into a symbol library file. Importing a symbol Part Menu 1 From the Part menu, select Import to display the Import dialog box. 2 In the File Name text box, type the name of the file to be imported, or select the file name from the file selection list.
Creating New Symbols 2 In the Part Name text box, enter the name of the symbol to be exported, or select it from the list. 3 In the File Name text box, enter the name of the file to which the part definition is to be written. 4 Click OK. Using AKO Symbols Some of the Orcad symbol libraries are made up of a few base symbols and several AKO (A Kind Of) symbols. In the bipolar.slb symbol library, for example, the qnpn and qpnp symbols are base symbols.
Chapter 6 Creating and Editing Symbols 2 Enter a name for the part in the Part Name text box (TestCase, for example). 3 Enter a description of the part in the Description text box. 4 Leave the AKO Name text box blank, and select Do not display in the Part Browser check box. 5 Click OK. Saving the symbol to a library 1 From the File menu, select Save. 2 In the File Name text box, type the name of the library. 3 Click OK.
Creating New Symbols Creating an AKO symbol 1 From the Part menu in the symbol editor, select New. 2 In the Part Name text box, type a name for the part. 3 In the Description text box, type a description of the part. 4 In the AKO Name text box, type the name of the base symbol (or example, AKO Test). 5 Click OK. The symbol graphics of the base symbol display in the symbol editor window. Select Save from the File menu to save the custom symbol library.
Chapter 6 Creating and Editing Symbols Drawing Symbol Graphics There are several graphics tools available for drawing symbols. With these tools you can draw circles, lines, arcs, and boxes. You can also place pins and text on your symbol. The default properties of the individual display layers, such as colors, line width, and style are set in the Display Preferences dialog box.
Drawing Symbol Graphics 2 Click at the location for the upper-left corner of the box. 3 Move the pointer down and to the right. A dotted box outline follows the pointer. 4 Click to set the lower-right corner of the box. Circle Drawing a circle 1 Click the Draw Circle button to change the pointer to a pencil shape. 2 Click the location of the center of the circle. 3 Move outward from the center of the circle. A dotted circle outline follows the pointer.
Chapter 6 Creating and Editing Symbols Adding arrowheads to polylines If you decide you don’t want to apply the changes you have made, click the Restore Defaults button to restore the settings selected in the Display Preferences dialog box. The Restore Defaults button works at any time before closing the dialog box or after re-entering it. 1 Select one or more polylines. 2 From the Edit menu, select Graphics Properties. 3 Select the appropriate arrowhead properties. 4 Click OK.
Drawing Symbol Graphics An outline box follows the pointer that indicates the outline of the text string. 4 Move the outline to the desired location and click to place the text. The outline box remains on the screen. You can click to place the same text string in several locations. 5 To stop placing the text string, do one of the following: • Double-click to place the last instance of the text. • Right-click to stop placing the text string without placing an additional one.
Chapter 6 Creating and Editing Symbols Selecting Selecting an element of a drawing 1 Click to select the element. The object color (the default is set in the Display Preferences dialog box) indicates it is selected. 2 Move or edit the object as necessary. Selecting a new object causes any previously selected items to be unselected. Selecting more than one element selection rectangle 1 Hold down S while selecting the elements. The selected elements change color.
Drawing Symbol Graphics Filling Shapes Shapes that have been drawn using either the schematic editor or the symbol editor may be filled with color. In the symbol editor you can fill circles, rectangles, and polylines. Use the Graphics Properties dialog box to change properties on an instance basis, but use the Display Preferences dialog box to set the defaults of those properties (see Changing Graphics Properties on page 4-131). Filling a shape after it has been drawn 1 Select one or more shapes to fill.
Chapter 6 Creating and Editing Symbols Ordering Drawing Objects When you draw or paste an object in the symbol editor, PSpice Schematics places it in front of all other objects on the page or in a graphics frame. If the object is filled, it can obscure other objects. You can control how objects overlap by putting them in front or in back of other objects. Moving objects in back of other objects 1 Select the object you want to place behind another object.
Drawing Symbol Graphics Rotating and Flipping Elements In the symbol editor, you can rotate and flip (mirror) elements currently being drawn, elements already drawn, and entire areas of a drawing. A rotated element is rotated 90° counter-clockwise. A flipped element is mirrored about the Y-axis. Rotating and flipping must occur during one of the following: • while dragging (before placement) • after placement Rotating Elements Rotating an element before placing it 1 Select an element to be placed.
Chapter 6 Creating and Editing Symbols Flipping a Drawing Element Flipping Elements Flipping an element before placing it on the drawing 1 Default Flipped once 186 Press C+F to flip the element, while still in the drag mode. Flipping an already placed element 1 Select the element. 2 Press C+F to flip it. Flipping an area of the drawing 1 Drag the mouse to select and outline the area to be flipped. 2 Press C+F to flip the area about its vertical axis.
Drawing Symbol Graphics Moving Moving an object 1 Select an object (or group of objects). 2 Place the pointer on the edge of the object or selected area and the annotation movement cursor becomes attached to the pointer. 3 Drag and place the object at the desired location on the page. Resizing Objects that have already been drawn can be resized by using the appropriate handles. Resizing an object 1 Select the object that you want to resize.
Chapter 6 Creating and Editing Symbols Editing Existing Symbols To edit an existing symbol, you must first load the library that the symbol is stored in. After the symbol is loaded, it can be edited by using all of the common editing functions that are available. To edit packaging information for a symbol, see Editing a Package Definition on page 6-204. Accessing Symbols Loading a symbol library 1 Click the File Open button on the toolbar. 2 Type a library name in the Open dialog box. 3 Click OK.
Editing Existing Symbols Cutting, Copying, and Pasting The symbol editor has editing functions to cut, copy, paste, repeat, delete, and undelete selected objects. These functions are available under the Edit menu, or can be accessed with keyboard shortcuts. The cut, copy, and delete functions apply only to selected objects. See Selecting on page 6-182 to learn how to select single and multiple objects as well as objects within a given area.
Chapter 6 Creating and Editing Symbols Pasting Paste places one or more copies of the last object stored in the buffer (from a cut or copy operation) onto the drawing. Pasting an object Shortcut: press C+V 1 From the Edit menu, select Paste to change the pointer to the shape of the object that was last cut or copied. 2 Click to place the object on the schematic. Continue moving the pointer to various locations and clicking to place additional copies of the object.
Defining and Editing Pin Types Defining and Editing Pin Types Pins establish the input and output terminals for symbols. For a pin you can: • select the type of graphic to display. • specify a pin name. • specify a pin number. • choose to display the name, the number, or both. Specifying Pin Types Figure 18 shows the twelve types of pins that you can place using PSpice Schematics.
Chapter 6 Creating and Editing Symbols Changing the type of a placed pin You can also double-click the pin to display the Change Pin dialog box. 1 Select the pin and from the Edit menu, select Change. 2 In the Type list box, select a pin type. 3 Click OK. The Float= and Modeled Pin boxes in the Change Pin dialog are only relevant for symbols that are going to be simulated with PSpice. For additional information, refer to your PSpice user’s guide. The change is only in effect for the selected pin.
Defining and Editing Pin Types Displaying the pin name By default, pins you place on symbols will have their pin names displayed. To disable pin names, do the following: 1 Double-click the pin or pin name to display the Change Pin dialog box. 2 Select the Display Name check box to disable the name display. 3 Click OK. Displaying the pin number By default, pins you place on symbols will have their pin numbers displayed.
Chapter 6 Creating and Editing Symbols Defining and Editing Hidden Power and Ground Pins If you set the visibility off, you must supply the name of a connecting net (typically a global net like $G_DPWR or $G_DGND) for the pin in the Net text box. With the symbol editor, you can set a pin to be invisible. If you set the visibility off, you must supply the name of a connecting net (typically a global net like $G_DPWR or $G_DGND) for the pin in the Net text box.
Defining and Editing Pin Types Changing Symbol Origin and Bounding Box The origin is designated for placing a part, and is the point the part is rotated around. By default, the origin is at (0,0). It is maintained as a point of reference on the schematic. The bounding box defines the selection area of the symbol when placed on a schematic. After drawing a symbol, all of the elements of the symbol must be enclosed in the bounding box.
Chapter 6 Creating and Editing Symbols Bounding Box • All pins must be contained within the bounding box for proper connections to be made in the schematic editor. • Hidden pins, like those found on digital parts, do not have to be, and in most cases are not, contained within the bounding box. • Attributes do not need to be contained The bounding box is the rectangular dotted line surrounding the symbol.
Editing Symbol Attributes Editing Symbol Attributes You can add attributes (properties) to a symbol. When you add an attribute, you specify a name and a default value. This value can be changed when the symbol is used on a schematic. You can specify whether or not to display the attribute. There are two attributes that are automatically added to symbols that are created. • The REFDES attribute, whose default value is U?, specifies the reference designator pattern to use in the schematic editor.
Chapter 6 Creating and Editing Symbols 198 2 In the Name text box, type the name of the attribute. 3 Optionally, type in the default value in the Value text box. 4 By default, the attribute Value only displays on the symbol. To disable any display, select None in the What to Display frame. 5 By default, the attribute value can be changed in the schematic editor on an instance-by-instance basis.
Editing Symbol Attributes Editing a displayed attribute 1 Double-click the displayed attribute. To edit an undisplayed attribute, or to make multiple changes, click the Edit Attributes button on the toolbar.
Chapter 6 Creating and Editing Symbols Using Symbol Aliases A symbol has a name. It can also have one or more aliases associated with it. Aliases are alternative names that the device represented by the part are known by. For example, you can have a symbol named 74AC269, which has as one of its aliases HD74AC269P. When defining an alias, keep in mind that the aliased device will share the same graphics, pins and attributes as the primary symbol.
Specifying Part Packaging Information Specifying Part Packaging Information If you are going to use a symbol for PCB layout, you will need to specify package or device information.
Chapter 6 Creating and Editing Symbols Packaging Definitions Packaging information is kept in a package definition, separate from the symbol definition. Both are maintained using the symbol editor. By default, the name of the package definition for a symbol corresponds to the symbol name. This can be overridden by explicitly adding a COMPONENT attribute to the symbol.
Specifying Part Packaging Information Copying a Package Definition With the Copy function in the Packaging menu, you can create a new package definition from an existing one. It is the same as the Copy function under the Parts menu, the definition may be copied from the active library or a different library. See “Making a Copy of a Symbol” on page 173. Copying a package definition 1 From the Packaging menu, select Copy to display the Copy Package Definition dialog box.
Chapter 6 Creating and Editing Symbols Editing a Package Definition You can edit a package definition for the active symbol or for any package definition in the open package library. Editing the package definition for the active symbol 1 From the Package menu, select Edit to display the Package definition dialog box. The options within the dialog box are discussed in the following sections. 2 Packaging Menu When you are finished with the dialog box, click OK.
Specifying Part Packaging Information 2 Click Edit Package Types to display the Edit Package Types dialog box. 3 In the Package Types per Pin Assignment text box, type the name of the package (for example, DIP14) or select a type from the Configured Package Types scroll list. 4 Click Add. 5 Click OK. 6 In the Package Definition dialog box, click OK. Note The Configured Package Types List is a list of commonly used package types; it is not an exhaustive list.
Chapter 6 Creating and Editing Symbols Specifying physical pin numbers For each package type (or group of package types that share the same pin-out) the physical pin numbers for each pin must be defined. The Pin Assignments frame in the Package Definition dialog box shows the pin numbers assigned for each logical pin on the symbol (for the active package type). Note The pin name must match that used in the symbol.
Specifying Part Packaging Information Any changes you make to a pin assignment are not in effect until you select Save Assignment. If you make a change to a pin and then select another pin from the list without saving, the changes are not implemented. 7 When you are finished editing pins, click OK. 8 In the Package Definition dialog box, click OK.
Chapter 6 Creating and Editing Symbols After you have defined the names of the gates, you must define pin numbers for each pin in each gate. On the symbol for the gate defined above, if there are any shared power pins, ground pins or both, you have to define them as hidden pins. 208 Defining pin number assignments 1 From the Packaging menu, select Edit to display the Package Definition dialog box (see 6-205). 2 Click Edit Pins to display the Pin Assignments dialog box (see 6-206). 3 In the Pin No.
Specifying Part Packaging Information Specifying Which Pins Can Be Swapped Pins within a gate that are logically equivalent to one another can be swapped. Pin swapping is usually done during layout to minimize the complexities of circuit routing. Enabling pin swapping 1 From the Packaging menu, select Edit to display the Package Definition dialog box (see 6-205). 2 Click Edit Pin Swaps to display the Pin Swaps dialog box. 3 In the Pin Names list, select two or more pins that you want to swap.
Chapter 6 Creating and Editing Symbols Creating Components With Multiple Gate Types Some components consist of two or more different types of gates (for example, ECL devices). Each type of gate will have a different logical symbol with a unique name, but reference the same package definition. For these types of components, you have to perform several additional steps in defining the package.
Specifying Part Packaging Information 6 Type a value in the Value text box corresponding to one of the gate types specified in the package definition. Example: For the 10102NOR symbol, GATETYPE = 1 (gates A,B,C); for the 10102ORNOR symbol, GATETYPE = 2 (gate D). 7 Click Save Attr. 8 Click OK to exit the dialog box.
Chapter 6 Creating and Editing Symbols Configuring Package Types When you create package definitions and specify package types for a device, you can pick from a list of commonly used package type names or enter one of your own. To add to the list of commonly used package type names that are presented, use the Configure Package Types selection from the Packaging menu. Also use this selection to configure package types into the package classes that are used when you package a design.
Specifying Part Packaging Information b Type in the name of the new class in the Package Class text box. c Click Add. d Click OK. 4 Click Add. 5 Click OK.
Chapter 6 Creating and Editing Symbols Configuring Custom Libraries When you create a library, whether it is a library of symbols or a library of packaging information, the symbols and packaging information are not available for use in the schematic editor until the library is configured. Configuration consists of adding the library file to the list of configured files.
Configuring Custom Libraries b Type the name of the one you are adding in the Library Name text box. Be sure the appropriate check boxes are selected to indicate whether you are configuring just the symbol library, or the symbol and package library. 6 Click Add. 7 Click OK. Note You may need to modify the Library Path (in the upper-right corner of the Editor Configuration dialog box) to include any directory paths that contain library files you added in the previous dialog.
Chapter 6 Creating and Editing Symbols Example—Creating Symbols from Scratch You can create custom symbols from scratch in PSpice Schematics.
Example—Creating Symbols from Scratch Figure 19 Example of Diode Bridge Rectifier Symbol Opening or Creating a Symbol Library To open or create a symbol library 1 In the schematic editor, from the File menu, select Edit Library to open the symbol editor. 2 To add this symbol to an existing symbol library: 3 a From the File menu, select Open. b Navigate to your file and open it. Note that the file status is : (at the top of the window). This means it is a new file (and a new symbol).
Chapter 6 Creating and Editing Symbols This example does not use AKOs or aliases. • The type of the part—the part type is most commonly “component,” as it is in this example. • An AKO or alias—use AKO if you want it to inherit the graphics and attributes from another symbol. Use Alias to assign additional names that this symbol can be used for. Drawing the Graphics After the symbol has a definition, the next step is to draw the graphics.
Example—Creating Symbols from Scratch e 4 Draw a line at a 45-degree angle across the right angle of the symbol already created to denote the cathode. Place three copies of this diode: a Drag the mouse to select the area that includes the graphics. Release the mouse to turn the lines red. If they do not turn red, reselect the area, or S+ click the unselected items to add them to the selected group. b From the Edit menu, select Copy. c From the Edit menu, select Paste.
Chapter 6 Creating and Editing Symbols Placing Pins To place pins You can also click the pin to change the name. 1 From the Graphics menu, select Place Pins. 2 To place the pins: 3 a Place the IN+ and IN- pins as shown in Figure 19. b Press C+ R to rotate the pin that is attached to the cursor. c Place the OUT+ and OUT- pins as shown in Figure 19.
Example—Creating Symbols from Scratch 3 From the Graphics menu, select Draw Text to place the labels D1 through D4 on the diode symbols. 4 To change the size of the text, double-click the text and adjust the size. The number is a percentage relative to the usual size. 5 6 From the Graphics menu, select Box and click once to attach the bounding box to the cursor. a Move the cursor to the lower right so that the bounding box encloses the entire symbol.
Chapter 6 Creating and Editing Symbols 2 MODEL and TEMPLATE are only required if you are going to simulate. 3 4 Click PART. a Set its value to the name that you used in the original definition box. b Click Save Attr. Click MODEL. a Set its value to the same value as in your model or subcircuit definition. b Click Save Attr. Click TEMPLATE. The TEMPLATE attribute is the template for generating the netlist entry for this device.
Example—Creating Symbols from Scratch Configuring the Models The diode bridge symbol is now ready for use in PSpice Schematics, but the model library must also be configured if the design is going to be simulated. 1 From the Analysis menu, select Library and Include Files. 2 If the required library is not already in the Library section, click Browse. 3 Locate the library and click Open to put the library with its path in the File Name field. 4 Select either Add Library* or Add Library.
Chapter 6 Creating and Editing Symbols 224
Creating and Editing Hierarchical Designs 7 Overview This chapter explains the procedures for creating and editing a hierarchical design. Many of the procedures used for creating and editing a hierarchical design are the same as those for creating and editing a design as explained in Chapter 4, Creating and Editing Designs.
Chapter 7 Creating and Editing Hierarchical Designs Setting Up Multiple Views on page 7-237 describes how to set up and use alternate representations for a hierarchical block or symbol. Navigating Through Hierarchical Designs on page 7-239 describes how to move between pages in a hierarchical design. Assigning Instance-Specific Part Values on page 7-241 describes how to assign instance-specific parts values.
Hierarchical Design Methods Hierarchical Design Methods You can create a hierarchical drawing in either of two ways: • Create a block and later assign a schematic to the block (top-down method). • Create a schematic and turn it into a symbol to be used in a higher level design (bottom-up method). Hierarchical design is a useful way to structure large projects, especially those starting from a block diagram and those with multiple occurrences of common circuitry.
Chapter 7 Creating and Editing Hierarchical Designs Creating and Editing Hierarchical Blocks A hierarchical block represents a collection of circuitry in the form of one or more lower-level schematics. The block displays on a schematic as a rectangle with a variable number of input and output ports. You can place one or more instances of a hierarchical block on a schematic. After you place a block, you can stretch it, reshape it and move it.
Creating and Editing Hierarchical Blocks Changing the reference designator of the hierarchical block 1 Double-click the HBn reference designator to display the Edit Reference Designator dialog box. 2 Type the reference designator in the Package Reference Designator text box. 3 Click OK to close the dialog box. The block, as placed, is a standard size, orientation and shape. You can stretch and reshape the block. Resizing a hierarchical block 1 Select the block to display its handles.
Chapter 7 Creating and Editing Hierarchical Designs The Implementation frame in this dialog will only display if you are using Design Lab. Note Interface input and output ports are created automatically only the first time you push into the block. Thereafter, you must manually add any additional interface input and output ports. 3 Type the new schematic name. 4 Click OK. A new schematic displays and contains interface input and output ports corresponding to the pins connected to the block.
Creating and Editing Hierarchical Blocks Editing a pin name on a hierarchical block 1 Select the pin on the hierarchical block. 2 Click the Edit Attributes button to display the Change Pin dialog box. 3 Type the desired pin name in the Pin Name text box. 4 Click OK. Double-click the pin to achieve the same results as steps 1 and 2. Deleting a pin on a hierarchical block 1 Select the pin. 2 Press D.
Chapter 7 Creating and Editing Hierarchical Designs Associating an Existing Schematic Instead of pushing into the block to create a schematic (see 7-229), you can associate an existing schematic with a hierarchical block. Associating an existing schematic with a hierarchical block You can also double-click the block to display the Set Up Block dialog box. 1 Select the Draw block button. 2 Place the block and be sure it stays selected.
Creating and Editing Hierarchical Symbols Creating and Editing Hierarchical Symbols PSpice Schematics uses two basic types of symbols: primitive and hierarchical. Primitive symbols are low level symbols that explicitly contain all of the information required by the netlister. They can be modified by editing their graphics, pins, and attribute lists in the symbol editor. Most of the symbols provided in the PSpice Schematics symbol libraries are primitive.
Chapter 7 Creating and Editing Hierarchical Designs connected to, is created for each hidden pin. Hidden pins are especially useful for global power and ground on digital parts ($G_DPWR, $G_DGND). File Menu Symbolizing a schematic 1 Open the schematic. 2 From the File menu, select Symbolize to display the Save As dialog box. 3 Type the name of the symbol. 4 Click OK. A file selection dialog box prompts for a symbol library to save the symbol in.
Creating and Editing Hierarchical Symbols Converting Hierarchical Blocks to Symbols When you finish editing a hierarchical block, you have the option of turning the block into a symbol. By making the block a symbol, you make it available for use in other schematics. Converting a block to a symbol 1 Select the block. 2 From the Edit menu, select Convert Block to display the Save As dialog box. 3 Type a name for the symbol. 4 Click OK to display the Open dialog box. 5 Select a library.
Chapter 7 Creating and Editing Hierarchical Designs Using Interface Ports When you use a block or symbol to represent an underlying schematic, connections to the underlying schematic are made by means of the pins on the block or symbol. The pins on the block or symbol must correspond to interface ports placed on the underlying schematic, that is, for each pin there must be a corresponding interface port with the same name as the pin.
Setting Up Multiple Views Setting Up Multiple Views A view is an underlying representation of a hierarchical block or symbol. A block can have more than one underlying representation by having multiple views. For example, you can define a part that has a transistor-level schematic as one view and a behavioral model schematic as another view. Note There are no restrictions on how many views a part can have, or on what the views are. Hierarchical symbols have one or more views.
Chapter 7 Creating and Editing Hierarchical Designs Setting up an associated view for the Translator Options Menu 238 1 From the Options menu, select Translators to display the Translators dialog box. 2 Select a Translator from the list or type a name in the Translator text box. 3 Type the name of the view in the View text box. 4 Click Apply. 5 Click OK.
Navigating Through Hierarchical Designs Navigating Through Hierarchical Designs The Navigate menu has functions that enable you to move between pages, create new pages, delete pages, and copy pages. You can move within a hierarchical design using functions from the Navigate menu. You can push into a block from the schematic, move up and down in hierarchical levels and identify the hierarchical path of a selected symbol. Moving down in a hierarchy 1 Select the hierarchical block or symbol.
Chapter 7 Creating and Editing Hierarchical Designs Finding where active schematic fits in a hierarchy Navigate Menu 1 From the Navigate menu, select Where to display the Where dialog box. The dialog box shows where the open schematic fits in the hierarchy of the open design. 2 240 Click OK.
Assigning Instance-Specific Part Values Assigning Instance-Specific Part Values The Edit Schematic Instance function enables you to view and edit the instance specific attributes associated with the instance of the block or hierarchical symbol that you pushed into. You can only add, change, or delete attributes when this function is activated. Any changes only apply to this instance of the hierarchical block or symbol.
Chapter 7 Creating and Editing Hierarchical Designs Passing Information Between Levels of Hierarchy With PSpice Schematics, you can create a lower-level schematic such that different instances of it will have different component values. For instance, a lower-level schematic contains a certain resistor. The hierarchical block or symbol representing the lower-level schematic defines the value of the resistor.
Passing Information Between Levels of Hierarchy found at that level, PSpice Schematics then searches the parent level. It continues up the hierarchy until it either finds a definition or until it reaches the top of the hierarchy. • When PSpice Schematics finds an attribute, it evaluates the attribute at the level where it is found. If the attribute value refers to other attributes, those other attributes must exist at the present level or higher in the hierarchy.
Chapter 7 Creating and Editing Hierarchical Designs Example—Creating a Hierarchical Design This example shows you how to create schematics from the top level down. The design consists of a simple schematic with a block representing a CMOS inverter and a lower-level schematic for the inverter. Follow this example to create the top-level circuit shown in Figure 20 and the inverter schematic shown in Figure 21.
Example—Creating a Hierarchical Design Placing the voltage source 1 Click the Get New Part button to display the Part Browser dialog box. Note One of two Part Browser dialog boxes may appear: the Part Browser Advanced and the Part Browser Basic. The advanced browser contains many features that you don’t need to use for this example. If the Part Browser Advanced dialog box appears, click <
Chapter 7 Creating and Editing Hierarchical Designs 6 Enter CMOSINV in the text box. This changes the value of the REFDES attribute from HB1 to CMOSINV. 7 Click OK. Drawing the output load resistor 1 Click the Get New Part button to display the Part Browser dialog box (see 7-245). 2 Type R in the Part field. 3 Click Place & Close. 4 Press C+R to rotate the resistor symbol. 5 Move the resistor symbol to the desired location. Click to place the symbol. 6 Right-click to stop placing parts.
Example—Creating a Hierarchical Design Wiring the Symbols Now that you have placed all of the symbols, wire the symbols to look like the schematic shown in Figure 20. 1 Click the Draw Wire button to change the pointer to a pencil. 2 Click the top of V1. Click at the location of the wire vertex (where it turns from the vertical to the horizontal). Click the left side of the CMOS block. The wire is complete when it shows connection on both ends.
Chapter 7 Creating and Editing Hierarchical Designs Saving your work as a top-level schematic 1 Click the Save File button. 2 Type tlcmos as the name of the file (the .sch extension is assigned by default). 3 Click OK. Drawing the Lower-Level Schematic The top-level design is complete. Now you can create the inner schematic of the CMOS inverter. To do so, select the block and use the Push selection from the Navigate menu to push to a lower level.
Example—Creating a Hierarchical Design Selecting the block and naming the new schematic 1 Click the CMOSINV block to select it. 2 From the Navigate menu, select Push. Because the block is new, the Setup Block dialog box appears. 3 Enter the new schematic name, cmos. 4 Click OK. 5 Move the interface port symbols in the same way you move other symbols: a Click to select it. b Drag it to the desired location. c Release to complete the move.
Chapter 7 Creating and Editing Hierarchical Designs 6 Right-click to stop placing parts. 7 Click the Get New Part button to display the Part Browser dialog box (see 7-245). 8 Enter M2N6802 in the Part text box. 9 Click Place & Close. 10 Move the part symbol to the desired location of M2 and click to place the part. 11 Right-click to stop placing parts.
Example—Creating a Hierarchical Design Drawing the wires Click the Draw Wire button and draw wires to connect parts and symbols as shown in Figure 21. Saving the file Click the Save File button to save the schematic. You are not prompted for a file name because the schematic was named when you pushed into it from the top-level schematic.
Chapter 7 Creating and Editing Hierarchical Designs 252
Preparing Your Design for Simulation 8 Overview This chapter provides guidelines for preparing your schematic for simulation and references further information contained in your PSpice user’s guide. A design that is targeted for simulation will have: • parts that there are simulation models available and configured for (Refer to Linking a Symbol to a Model or Subcircuit Definition in your PSpice user’s guide.
Chapter 8 Preparing Your Design for Simulation Editing Simulation Models from PSpice Schematics on page 8-258. Adding and Defining Stimulus on page 8-259. Starting the Simulator on page 8-266. Viewing Results on page 8-267.
Creating Designs for Simulation and Board Layout Creating Designs for Simulation and Board Layout When creating designs for both simulation and printed circuit board layout, some of the parts you use will be for simulation only (for example, simulation stimulus parts like voltage sources), and some of the parts you use will have simulation models that only model some of the pins of the real device.
Chapter 8 Preparing Your Design for Simulation Handling Unmodeled Pins Parts that have some pins that are not modeled, will appear broken when placed on the schematic. To see an example of this, place an instance of the PM-741 part from the “opamp.slb” symbol library. The OS1 and OS2 pins are not modeled, so only the +, -, V+, V-, and OUT pins are netlisted for simulation. For the simulator, these pins appear as a large resistor connected to the ground.
Specifying Simulation Model Libraries Specifying Simulation Model Libraries Refer to the Creating Models chapter of your PSpice user’s guide for information about creating and configuring simulation model libraries. Each part that you intend to simulate must have a simulation model defined. Checking if a part has a simulation model defined Double-click the part on the schematic to display the Attribute Editing dialog box.
Chapter 8 Preparing Your Design for Simulation Editing Simulation Models from PSpice Schematics You can define and edit simulation models directly from PSpice Schematics. Models can be defined using the Parts utility or the text editor (sometimes called the Model Editor). The Parts utility is useful for characterizing specific models from data sheet curves.
Adding and Defining Stimulus Adding and Defining Stimulus The Stimulus Editor is a utility that enables you to set up and verify the input waveforms for a transient analysis. You can create and edit voltage sources, current sources, and digital stimuli for your circuit. Menu prompts guide you to provide the necessary parameters, such as the rise time, fall time, and period of an analog repeating pulse, or the complex timing relations with repeating segments of a digital stimulus.
Chapter 8 Preparing Your Design for Simulation Setting Up Analyses Refer to your PSpice user’s guide for information about setting up and running the many different analysis types supported by PSpice A/D. Creating a Simulation Netlist Overview A netlist is the connectivity description of a circuit, showing all of the components, their interconnections, and their values. When you create a simulation netlist from Schematics, that netlist describes the current design. For Release 9.
Adding and Defining Stimulus Note For Release 9.2, the maximum limits have been removed for the following .SUBCKT arguments: nodes, parameters, and optional nodes. Hierarchical netlists are especially useful to IC designers who want to perform Layout vs. Schematic (LVS) verification because they are more accurate descriptions of the true circuit. Using netlisting templates In Schematics, the template property specifies how primitive parts are described in the simulation netlist.
Chapter 8 Preparing Your Design for Simulation For Release 9.2, markers can now be placed on subcircuit nodes as well. This allows you to perform cross-probing between Schematics and PSpice at the lower level circuits of a hierarchical design. Note If conditional constructs are used, the hierarchical netlist will create a unique subcircuit definition for each instance. Creating the netlist You can generate a flat or hierarchical simulation netlist (.
Adding and Defining Stimulus 3 If you want the .PARAM commands to be made global in scope, check the Make .PARAM Commands Global checkbox. If this is disabled, the param symbols will be local to the subcircuit in which they occur. 4 Click OK. Note To save the current settings and make them become the default settings for use later, click the Save as Default button. Creating an LVS netlist {bmct NEW.BMP} To create an LVS netlist 1 Note From the Tools menu, choose Create LVS Netlist.
Chapter 8 Preparing Your Design for Simulation Note The LVS netlist is written in general syntax and should be compatible with most LVS tools. Depending on the tool you intend to use, however, you may need to modify the file in particular ways in order for it to be usable with your specific system. Specifying alternate netlist templates To specify an alternate netlist template 1 From the Options menu, choose Netlist Setting. The Netlist Setting dialog box appears.
Adding and Defining Stimulus Use the control buttons located directly above the Use Template list box to configure the list of templates. You can: Note • add a new template by clicking the New icon or by double-clicking in the dashed box at the beginning of the list. • delete a template by selecting the name and then clicking the Delete icon. • edit a template name by selecting the name and then clicking the Edit icon.
Chapter 8 Preparing Your Design for Simulation 4 With the SUBPARAM part still selected, from the Edit menu, choose Attributes. 5 In the Attributes dialog box, define the names and default values for the attributes that can be changed on an instance-by-instance basis. 6 In the top-level schematic, use the Attributes dialog box to edit the attributes of the hierarchical part or block that references the subcircuit (child) schematic so they match the attributes you defined in Step 5.
Viewing Results Viewing Results You can use Probe to view and perform waveform analysis of the simulation results. For more information, refer to the Waveform Analysis chapter of your PSpice user’s guide. View Probe Help for more information. Viewing Bias Point Results After simulating, you can display bias point information on your schematic so that you can quickly zero in on problem areas of your design. PSpice A/D calculates and saves the bias point voltages and currents.
Chapter 8 Preparing Your Design for Simulation Using Markers You can place markers on your schematic to indicate the points in Probe where you want to see waveforms displayed. Note For Release 9.2, markers can now be placed on subcircuit nodes as well. This allows you to perform cross-probing between Schematics and PSpice at the lower level circuits of a hierarchical design.
Viewing Results Configuring Probe Display of Simulation Results To configure what Probe displays when it is started, select Probe Setup from the Analysis menu. You are given the following choices: • Restore Last Probe Session—This restores the display characteristics from the last session of Probe. • Show All Markers—This displays the waveforms at the points on the schematic that have been marked by markers.
Chapter 8 Preparing Your Design for Simulation 270
Using Design Journal 9 Overview This chapter provides introductory information about the Design Journal. In this chapter you will find the following sections: Understanding Design Journal on page 9-272 describes the purpose and different uses of Design Journal. Design Journal Help on page 9-273 describes where to find Design Journal Help.
Chapter 9 Using Design Journal Understanding Design Journal Design Journal is a very powerful analysis and tracking tool.
Design Journal Help working schematic (MySchem) 1st checkpoint schematic (Checkpoint.001) 2nd checkpoint schematic (Checkpoint.
Chapter 9 Using Design Journal 274
Preparing Your Design for Board Layout 10 Overview This chapter describes how to prepare your design for use with a board layout program and has the following sections: Connectors on page 10-277 describes placing connectors to provide the interface between the PCB and the rest of the system. This section also describes how to create connector symbols.
Chapter 10 Preparing Your Design for Board Layout Interfacing to Board Layout Products on page 10-292 describes the procedures for using PSpice Schematics with the board layout products from other vendors.
Connectors Connectors Connectors provide the interface between a PCB and the rest of a system. The distinction between connectors and ports on a schematic is important and is shown in Table 14. Off-page ports are not physical connectors, so you cannot use an off-page port as a connector or a connector as an off-page port. You may use them together if you want to have both connectivity and a physical part by attaching an off-page port to the pin of the connector.
Chapter 10 Preparing Your Design for Board Layout Using Connector Symbols that Represent the Entire Connector These symbols will have as many pins as the physical connector they represent. You can wire signals directly to the pins or connect labeled off-page (or global) ports to each pin. The label indicates the signal name that will be connected to the pin. Any off-page ports in the design with that same signal name will be connected to that connector pin.
Connectors Creating Single-Pin Connector Symbols When creating a connector pin symbol, you must correctly define the connector package for the layout netlist to be correct. For example, in creating a 62-pin edge connector, instead of creating a single symbol for a 62-pin edge connector with all 62 pins, you can create a symbol of a single connector pin and attach to it PKGREF and GATE attributes (created and assigned when the symbol is placed).
Chapter 10 Preparing Your Design for Board Layout Packaging the Parts in Your Design Symbols used in PSpice Schematics represent either an individual gate of a packaged device, or a complete device. When a symbol representing a single gate is placed on a schematic, it is assigned a unique reference designator (if Auto-Naming is enabled), and by default, is made the first gate in the package.
Packaging the Parts in Your Design Pin numbers for devices with package definitions are determined from the package definition rather than from the symbol. • Pin numbers are dependent on the gate (for multi-gate parts) and package type (for devices with alternative pin assignments based on package type). Until both GATE and PKGTYPE attributes are assigned values, no pin numbers are shown. • For single gate packages with no gate name (for example, blank instead of A) no GATE attribute value is required.
Chapter 10 Preparing Your Design for Board Layout 2 Type a new value in the Package Reference Designator text box. 3 Click OK. If you have other parts that you want to automatically package together, use the All Except User-Assigned option when you package the design. Automatically packaging at a later time Tools Menu 1 From the Tools menu, select Package to display the Package dialog box. 2 In the Set Values for area, click the All Except User-Assigned option button.
Packaging the Parts in Your Design Assigning Reference Designators Automatically Use the Package selection from the Tools menu to package individual parts into physical packages. Packaging and assigning reference designators 1 From the Tools menu, select Package to display the Package dialog box (shown on 10-282). 2 In the Function area, click the Package and Assign Reference Designators Only button.
Chapter 10 Preparing Your Design for Board Layout Setting Package Class Priorities Priorities can be set (for the packager) to use in determining which package type to assign when a part is available in more than one type. For example, you could specify that a DIP package type be used. If the part is not available in DIP, then it could assign SMT, and so forth. For details on adding package types and classes, see Configuring Package Types on page 6-212.
Packaging the Parts in Your Design 5 If you want to insert a class into the Class Priorities list, first select a class from the Package Classes list, then select an item in the Class Priorities list and click Insert. The package class is added to the list before the item selected in the Class Priorities list. 6 Click OK. 7 In the Package dialog box, click OK.
Chapter 10 Preparing Your Design for Board Layout Generating a Bill of Materials Report If you select a part in the Part Browser and the name you select is an alias (electrically equivalent) of the basic symbol name, the part you get will have the basic symbol name. It will not have the name you type, therefore, it will effect your Bill of Materials. A Bill of Materials report lists the quantities of each component type used in the design along with corresponding reference designators.
Generating a Bill of Materials Report Generating a Bill of Materials report 1 Select Reports from the File menu to display the Reports dialog box. 2 Click Display. File Menu The Bill of Materials dialog box appears and you can print, display, or save the report. Closing the Reports dialog box 1 Click Close. Printing and Saving the Report Printing a Bill of Materials report 1 If not already in the Reports dialog box, select Reports from the File menu. 2 In the Reports dialog box, click Print.
Chapter 10 Preparing Your Design for Board Layout Customizing the Format of the Report 1 Click Setup to display the Report Setup dialog box. 2 In the Format text box, type the attributes to be displayed in the report according to the following syntax: [descriptive text]@ where the ‘@’ sign indicates value substitution for the named attribute. Specify multiple attributes by using the preceding syntax in a comma-separated list.
Generating a Bill of Materials Report User Defined Component Information You can display user-specific component information (such as, costs and in-house part numbers) in the Bill of Materials report. The Bill of Materials report will take a component description file as input. The component description file (.cdf extension) is a user-created and maintained text file that contains component information such as cost, supplier name and in-house order numbers.
Chapter 10 Preparing Your Design for Board Layout The COST entries for 10K and 1K resistors would appear in the component description file as follows: R,RC05,R1,VALUE,10K R,RC05,R1,COST,.05 R,RC05,R2,VALUE,1K R,RC05,R2,COST,.03 Specifying user-defined component attribute descriptions 1 From the File menu, select Reports to display the Reports dialog box (shown on 10-287). 2 Click Setup to display the Report Setup dialog box (shown on 10-288).
Swapping Pins Swapping Pins To swap pins on a given gate, add a SWAP attribute with the value of the pin names of the two pins to be swapped. For example: SWAP=A B will swap pin A with pin B. Edit Menu Swapping pins 1 From the Edit menu, select Attributes to display the Attribute Editing dialog box. 2 In the Name text box, type SWAP. 3 In the Value text box, type A B. 4 Click Save Attr. 5 Click OK. Note A and B must be pin names, not pin numbers.
Chapter 10 Preparing Your Design for Board Layout Interfacing to Board Layout Products PSpice Schematics creates layout netlists in the formats shown in Table 15. Table 15 Supported Layout Packages and File Formats Package Layout Netlist ECO File PADS .pad .eco P-CAD .alt (none) Protel .pro .eco Tango .tan .eco CADSTAR .cdn .rin SCICARDS .upl .sif EDIF 2 0 0 .
Interfacing to Board Layout Products Creating a Layout Netlist 1 Note From the Tools menu, select Create Layout Netlist. If you are using the Orcad line of products, you will be preparing the netlist as input to Orcad Layout. Although Schematics does not generate a netlist file (.MNL) that is directly compatible with Layout, you can create a netlist file that Layout will be able to process.
Chapter 10 Preparing Your Design for Board Layout Layout Mapping Files When creating layout netlists, PSpice Schematics uses mapping files. These files let you customize the handling by the layout netlister of part, net, and package type names. Mapping files are text files that you can edit with any text editor. PSpice Schematics is shipped with mapping files containing defaults and sample entries. Mapping files exist for each of the supported layout formats. • .
Interfacing to Board Layout Products Common Syntax Each file (.xmp, .xnt and .xpk) consists of a number of lines. Empty lines and those starting with the ‘#’ character are ignored. Otherwise, a line consists of one or more comma-separated identifiers followed by either an AKO specification or a replacement string. An AKO (A Kind Of) specifier consists of the keyword AKO, followed by an identifier.
Chapter 10 Preparing Your Design for Board Layout Parts List Mapping (.xmp) After PSpice Schematics has found a matching rule in the map file for the COMPONENT or PART attribute of a part, it further processes the replacement string. This processing is similar to the processing of the TEMPLATE attribute of a part when a simulation netlist is created. Identifiers in the string prefixed by one of the characters ‘@,’ ‘?,’ ‘~,’ ‘#,’ and ‘`’ are treated as part attribute names.
Interfacing to Board Layout Products C101 CAP,10uF or C102 CAP,10uF,20% depending on whether or not a TOLERANCE attribute has been specified. The VALUE attribute must be defined; PSpice Schematics will issue a message if a capacitor has no assigned value. To support the case where the designer wishes to specify a particular capacitor type (for example, CAP\CR08\5G from the PADS library), the designer places an instance of a capacitor and then sets the COMPONENT attribute to CAP\\CR08\\5G.
Chapter 10 Preparing Your Design for Board Layout The following rules in the .xpk file will implement this: DIP* CC* -CC Note that the DIP* rule is empty; it matches package classes such as DIP14, but there is no resulting replacement string. The LCC* rule matches all strings that start with LCC, so it will match package classes such as LCC20 and LCC28. It appends the string -CC to the COMPONENT (or PART) name.
Interfacing to Board Layout Products Using back annotation 1 From the Tools menu, select Back Annotate to display the Back Annotate dialog box. 2 Type the name of the ECO file generated by the layout package in the ECO File Name text box. 3 Select an ECO file format from the ECO File Format list. 4 Click OK. Tools Menu In step 2, if you don’t know the file name, click Browse and select a file using the standard open file dialog box.
Chapter 10 Preparing Your Design for Board Layout 300
Exporting DXF Files A Overview This appendix provides information regarding exporting DXF files. In this chapter you will find the following sections: Exporting DXF Files on page A-302. Exporting from the Schematic Editor on page A-303. Exporting in the Symbol Editor on page A-304.
Chapter A Exporting DXF Files Exporting DXF Files The Export function generates Drawing Interchange Format (DXF) files. These files are also known as AutoCAD Format 2-D files. You can export the entire schematic drawing, a page, a portion of a page, or symbol graphics to a DXF file.
Exporting from the Schematic Editor Exporting from the Schematic Editor 1 From the File menu, select Export to display the Export dialog box. 2 Select one of the following options: • Click Select All to export all pages of the schematic file. • Select one of the entries in the Pages dialog box to export a specific set of pages. • Select the Selected Area Only check box to export the currently highlighted selection in the schematic editing area.
Chapter A Exporting DXF Files Exporting in the Symbol Editor File Menu To select more than one symbol, hold down S while selecting other pages. Note The Current Symbol Only option is only enabled if a specific symbol was selected in the drawing area before the Export menu item was chosen. 304 1 From the File menu, select Export to display the Export dialog box. 2 Select one of the following options: • Click Select All to export all symbols in the current symbol library.
Library Expansion and Compression Utility B Overview This Appendix explains the Library and Expansion Compression Utility that can be used with the PSpice Schematics libraries. In this chapter you will find the following sections: Using the Library Utility on page B-306. Expanding Library Definitions into Text Files on page B-307. Compressing Definition Files into a Library on page B-307. Salvaging a Corrupted File on page B-308. Reorganizing a Library File on page B-308.
Chapter B Library Expansion and Compression Utility Using the Library Utility PSpice Schematics includes a library utility (LXCWin) that works with the symbol, package, and footprint libraries. You can use LXCWin to: • expand a library into definitions and create a list of those definitions (.lst file) • compress definitions listed in the .
Expanding Library Definitions into Text Files Expanding Library Definitions into Text Files When you use LXCWin to expand a library, it reads the selected library line by line, and writes each definition of a symbol (.sym), package (.pkg), or footprint (.fpd) in plain ASCII format, to a text file. It also creates a .lst file, detailing the file name and the corresponding definition name. To expand a library into individual definition files: 1 From the Action frame, select Expand.
Chapter B Library Expansion and Compression Utility Salvaging a Corrupted File To salvage a corrupted file or one that has carriage returns and line feeds 1 In the Action frame, select Fix Index. 2 Click the Process File button. 3 Select a library. Reorganizing a Library File To reorganize a library file 1 Expand the library. 2 Edit the .lst file with a text editor to add, delete, or rearrange files. 3 Compress the library. .lst File Format Table 16 .
Running LXCWin Using Command Line Options Running LXCWin Using Command Line Options You can also run LXCWin using command line options. The options are: -f Fix Index (default) -x Expand -c Compress -n Do not delete definition files One or more library names; the names may include wildcards (*. ?) Example: LXCWin *.
Chapter B Library Expansion and Compression Utility 310
Advanced Netlisting Configuration Items C Overview This appendix contains information regarding advanced netlisting configuration. In this chapter you will find the following sections: Specifying PSpice Node Name Netlisting Preferences on page C-312. Specifying Board Layout Node Name Netlisting Preferences on page C-313. Customizing EDIF Netlists on page C-314.
Chapter C Advanced Netlisting Configuration Items Specifying PSpice Node Name Netlisting Preferences By default, the PSpice netlister assigns names such as $N_001 to nodes that are not explicitly labeled. You can change the format that the netlister uses to create these names by using a text editor and editing the pspice.ini file in the Windows directory.
Specifying Board Layout Node Name Netlisting Preferences Specifying Board Layout Node Name Netlisting Preferences To change any of these settings, use a text editor and edit the pspice.ini file in the Windows directory. PCBHIERPATHSEP is the separator character to use when creating hierarchal net names in layout netlisting. The PCBTEMPLATE item specifies the form that the layout netlister uses for creating node names.
Chapter C Advanced Netlisting Configuration Items Customizing EDIF Netlists You can change the amount each level in the netlist is indented by changing the EDIFINDENT item in the [SCHEMATICS] section of the pspice.ini initialization file. Use a text editor to edit the pspice.ini file in the Windows directory. EDIFINDENT specifies the character to use to indent each level in an EDIF netlist.
Attribute List D Overview This appendix is a list of attribute names used by PSpice Schematics and descriptions of each of those attributes.
Chapter D Attribute List provided as a default set. You can provide any other attributes as needed. Table 1 Reserved Attributes Attribute Description See Notes COMPONENT The name of the package definition to be used for a part. If the name of the package definition is the same as the part name, then the COMPONENT attribute is not necessary. 2 5 GATE The gate within the package that a particular part instance is assigned to.
Overview Table 1 Reserved Attributes (continued) Attribute Description See Notes MODEL The name of the model referenced for simulation. This name must match the name of the .model or .subckt definition of the simulation model as it appears in the Model Library file (.lib). For example, if your design includes a 2N2222 bipolar transistor, with the .model name Q2N2222, then the MODEL attribute on the symbol for that part will be Q2N2222.
Chapter D Attribute List Table 1 Reserved Attributes (continued) Attribute Description See Notes PKGTYPE The physical carrier type to be used for the part. (Examples: DIP14, LCC20, DIP8). If the package definition for the part has only one available package type defined, then the PKGTYPE attribute will be assigned this value. You can manually assign the package type by editing or creating this attribute, or you may have the PKGTYPE attribute assigned during packaging.
Overview Table 1 Reserved Attributes (continued) Attribute Description See Notes TEMPLATE The recipe for creating a netlist entry for simulation. The pin names specified in the TEMPLATE must match the pin names on the symbol. The number and order of the pins listed in the TEMPLATE must match those appropriate for the associated .model or .subckt definition referenced for simulation. The TEMPLATE attribute is only changeable in the symbol editor.
Chapter D Attribute List 320
Symbol Libraries E Overview This appendix contains the contents of the symbol libraries that are provided with PSpice Schematics.
Chapter E Symbol Libraries Using Symbol Libraries Symbols are stored in symbol libraries. The symbol library files have a .slb extension and contain graphical representations and attributes of parts. The contents of the symbol libraries provided with PSpice Schematics are listed in Table 2. Parts from libraries marked with † do not have corresponding simulation models.
Using Symbol Libraries Table 2 Symbol Libraries Symbol Library File Name Contents 7400.slb 7400-series TTL 74ac.slb Advanced CMOS 74act.slb TTL-compatible, Advanced CMOS 74als.slb Advanced low-power Schottky TTL 74as.slb Advanced Schottky TTL 74f.slb FAST 74h.slb High-speed TTL 74hc.slb High-speed CMOS 74hct.slb TTL-compatible, high-speed CMOS 74l.slb Low-power TTL 74ls.slb Low-power Schottky TTL 74s.slb Schottky TTL abm.slb Behavioral modeling blocks adv_lin.
Chapter E Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name Contents anlg_dev.slb Analog Devices Inc.: operational amplifiers, transistor arrays, buffers, voltage references, analog multipliers, analog switches apex.slb Apex Microtechnology Corporation: operational amplifiers atmel.slb† Atmel Corporation: EEPROM, PROM, SRAM, PLD bipolar.slb Bipolar transistors breakout.slb Parameterized devices for model purposes broktree.
Using Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name Contents dig_pal.slb Programmable array logic devices dig_prim.slb Digital primitives for use with PLSyn as well as general simulation purposes diode.slb Diodes, Zener diodes, current regulator diodes, varactors ebipolar.slb European bipolar transistors ecl.slb† Motorola Corp., National Semiconductor Inc.: DRAM, gates, multiplexers, level translators, prescalers, error correction/detection ediode.
Chapter E Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name 326 Contents hyundai.slb† Hyundai Electronic Inc. Ltd.: PLD, DRAM, SRAM intel.slb† Intel Corp.: EPROM, CPU, math co-processors, microcontrollers, SRAM, network processors jbipolar.slb Japanese bipolar transistors jdiode.slb Japanese diodes, rectifiers, Zener diodes, varactors, Schottky diodes jfet.slb Junction field-effect transistors jjfet.slb Japanese junction field-effect transistors jopamp.
Using Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name Contents misc.slb Timers, CMOS transistor arrays, variable admittance, variable impedance, three-phase transformers, relays, DC motor, time-dependent switches mitmem.slb† Mitsubishi Electric Corporation: EEPROM, PROM, DRAM, SRAM mitram.slb† Mitsubishi Electric Corporation: DRAM, SRAM mitrom.slb† Mitsubishi Electric Corporation: EPROM mix_misc.slb Timers, DC motors, relays mosel.slb† Mosel-Vitolic Inc.
Chapter E Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name 328 Contents nsucont.slb† National Semiconductor Inc.: microcontrollers oki.slb† OKI Semiconductor: display drivers, DRAM, EEPROM, EPROM, DRAM, SRAM, microcontrollers, clock, speech synthesis, recorders, CODEC, modems opamp.slb Operational amplifiers, voltage comparators, voltage regulators, voltage references opto.slb Opto couplers pansonc.slb† Panasonic Industrial Group: ROM, DRAM, SRAM, FIFO polyfet.
Using Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name Contents swit_rav.slb Averaged switched-mode power supply blocks swit_reg.slb Switched-mode regulators tex_inst.slb Texas Instruments Inc.: operational amplifier, voltage comparators thyristr.slb SCR, triac, UJT ti1.slb† Texas Instruments Inc.: line drivers, transceivers, display drivers, ADC, switches ti2.slb† Texas Instruments Inc.: SRAM, EPROM, DRAM, PROM, memory controllers tilsi.
Chapter E Symbol Libraries Table 2 Symbol Libraries (continued) Symbol Library File Name 330 Contents xicor.slb† XICOR Inc.: SRAM, EEPROM, potentiometers xtal.slb Quartz crystals zilog.slb† Zilog Inc.
Glossary ABM Analog behavioral model. A view of a hierarchical schematic used for analysis. See also View. AKO “A Kind Of” symbol. Symbols must either contain graphics or refer to an AKO symbol. The AKO defines the symbol in terms of the graphics and pins of another part. Both must exist in the same symbol library file. alias An exact electrical equivalent that can be used to reference a symbol.
Glossary May 16, 2000 bounding box bundle bus circuit connector current sensor A collection of named wires or buses of the same type or purpose. A collection of homogeneously named signals. A configuration of electrically connected components or devices. A physical device that is used for external connections to a circuit board. A connector has no electrical significance until it is connected on a PCB. Displays the bias point current flow in a given direction.
***Draft*** Glossary global port Provides a connection to another global port of the same name anywhere in the schematic. gravity The property of a drawing object to snap to the nearest grid or pin when being placed on a drawing or moved about a drawing. gravity radius The distance between the cursor and an object on the schematic in which the object can be selected.
Glossary May 16, 2000 navigation net netlist nodeset A set of electrically connected part pins. A net may be anonymous or named. An anonymous net might be the junction of two resistors. A named net could be a wire labeled CLOCK connecting two digital parts. A list providing the circuit definition and connectivity information in simulation netlist format. A symbol containing one or two pins, permitting you to initialize a node voltage for simulation.
***Draft*** Glossary part outline pin pin definition pin name pin number Consists of the symbol for a part (graphics and pins), minus any text. Contained in parts, ports and off-page connectors. Parts can contain multiple pins. Each part contains specific pin names associated with the part. Pins may connect to a wire, a bus or another pin. Provides the pin number, the location of each pin relative to the symbol origin and the electrical attributes of the pin.
Glossary May 16, 2000 selection area setpoint simulation stimulus symbol symbol definition When drawing or editing a schematic or symbol, the area identified and enclosed by a region-of-interest (ROI) box for the purpose of performing some operation on the objects within the area. A special symbol used to specify initial node voltages during simulation. The use of a mathematical model to represent the physical operation of a circuit design.
Index definition of, 331 specifier, 295 symbols, 175 A a kind of, See AKO ABM, 331 accessing symbols, 188 Add Text dialog box, 127 adding annotation graphics, 130 annotation text, 126 attributes, 90 library, 44 multiple line text, 126 non-electrical information, 126 package type, 212 package type for a component, 204 page to design, 136 pins to a symbol, 180 stimulus, 259 symbol alias, 200 text to schematic, 127 text to symbol, 180 wire segment, 104 Additional Info dialog box, 76 advanced netlisting confi
Index arc, drawing, 178 archive, 24 assigning annotation, 89 attribute names, 315 attribute value, 93 instance-specific part values, 241 pin numbers, 208 pins, 201, 206 reference designator, 14, 97, 228, 281 attribute definition of, 331 deleting, 90 editing, 88 enabling display, 91 global editing, 93 intrinsic property, 88 list, 315 non-changeable, 89 selecting, 116 simulation, 255 SWAP, 291 system defined, 89 text, 158 value, 30, 88 view, 237 Attribute Editing dialog box, 88 attribute text changing, 158 at
Index C CADSTAR layout format, 292 Change Attribute dialog box, 91, 158 Change Pin dialog box, 160, 192, 231, 247 Change Text dialog box, 161, 181 changing a placed pin type, 192 application settings, 64 attribute text, 158 attribute value, 93 border style, 52 bounding box size, 196 custom libraries, 94 default value, 94 display characteristics of attributes, 91 drawing area, 54 free-standing text, 161 graphics properties, 131–132 gravity, 55 grid, 55 hierarchical block reference designator, 229 library se
Index copying between pages, 138 package definition, 203 page, 137 part, 94 selected object, 189 symbol, 173 to clipboard, 121 Create Page dialog box, 136 creating AKO symbol, 177 annotation items, 126 annotation symbols, 134 base symbol, 175 connections between pages, 137 connector symbols, 279 custom title block, 124 design, 2 design for board layout, 255 design for simulation, 255 ground symbol, 103 hierarchical block, 228 hierarchical design, 2, 244 hierarchical symbols, 233 interface ports, 230 multipl
Index Back Annotate, 299 Block View, 232 Change Attribute, 91, 158 Change Pin, 160, 192, 231, 247 Change Text, 161, 181 Configure Tools, 292 Configuring Package Types, 212 Copy Package Definition, 203 Copy Page, 137 Copy Part, 94, 173 Create Page, 136 Definition, 200 Delete Page, 139 Display Options, 56–57, 110, 154, 162 Display Preferences, 62 Edit Attributes, 135, 291 Edit Gate Types, 207 Edit Package Definition, 202 Edit Package Types, 205 Edit Reference, 245 Edit Reference Designator, 14, 229, 281 Edito
Index drawing additional pages, 136 arc, 178 area, 54 block, 35 box, 178 bus, 12, 35, 106–107 circle, 179 connections, 107 custom power and ground symbols, 103 line, 179 lower-level schematic, 248 options, 109 orthogonal wires and buses, 109 symbol graphics, 178 text, 38, 127, 180 text box, 38, 126 top-level schematic, 244 wire, 11, 35, 104 DXF files exporting, 301 E ECO, 298 definition of, 332 file formats, 292 EDIF 2 0 0, 292 edit attributes, 160 Edit Attributes button, 35, 93, 155, 210, 231 Edit Attribu
Index associating with a hierarchical block, 232 Export file specification dialog box, 303 Export Parts dialog box, 174 exporting bill-of-materials report, 290 DXF Files, 301 from the schematics editor, 303 in the Symbol Editor, 304 symbol, 174 F file management, 19 opening, 33 saving, 33 fileset definition of, 332 filling shapes, 183 Find dialog box, 118 finding most recently placed part, 81 part, 80, 118 fitting view to page, 70 flat schematic definition of, 332 flipping area of drawing, 186 area of sche
Index navigating through, 239 passing information between levels, 242 hierarchical parts, 29 hierarchical symbol, 233 selecting, 239 horizontal offset, 96 hotspot definition of, 333 I Import dialog box, 174 Import OrCAD File dialog box, 303 importing annotation graphics, 133 bitmaps, 133 graphics, 181 in the schematic editor, 133 in the symbol editor, 181 into Microsoft Word, 121 metafiles, 133 symbol, 174 indicated severity of message, 74 insert picture, 181 Insert Picture button, 38, 133, 181 instance na
Index message definition of, 333 Message Viewer, 74 additional information, 76 closing, 76 severity indicator, 74 using, 73 metafiles importing, 133, 181 mirroring, See flipping model behavioral, 237 definition, 80 library, 80 name, 316 simulation, 256, 322 model definition definition of, 333 More Info button, 76 moving down in hierarchy, 239 interface port symbols, 230 non-electrical information, 135 object on schematic, 117 parts, 15 symbol element, 187 text, 15 to top of hierarchy, 239 up in hierarchy, 2
Index orthogonality, 109 printing, 140 scaling, 141 specifying gravity, 164 text grid, 165 origin, 195 definition of, 334 orthogonal connectivity, 109 drawing wires and buses, 109 enabling, 110 with rubberbanding enabled, 112 Outline border style, 53 P package definition of, 334 information, 201 library, 80 package class priorities, 284 package definition active symbol, 204 contents, 280 copying, 203 creating, 202 creating new, 202 deleting, 211 editing, 202 how used, 280 name, 316 open package library, 20
Index definition of, 334 part instance changing display of attributes, 91 definition of, 334 part origin editing, 195 part outline definition of, 335 part value, changing, 14 parts placing and editing, 85 stopping placement, 85 passing information between levels of hierarchy, 242 pasting between pages, 138 selected object, 119, 190 P-CAD layout, 292 pin adding to a symbol, 180 assignments, 205 broken, 256 definition of, 335 hidden, 31, 333 name, 160, 206 number, 160 shared power and ground, 208 snap to, 57,
Index properties changing, 128 Protel layout format, 292 pushing, 239 into block, 227 enabling, 113 orthogonal disabled with rubberbanding enabled, 112 with orthogonal enabled, 112 rules of connectivity, 106 R S Redraw button, 34, 39, 153, 155 reference designator assigning, 97, 281 auto-naming, 97 changing, 14, 229 definition of, 335 value, 318 refreshing the screen, 39 Remove Package Definition dialog box, 211 removing configured library, 46 package definition, 211 repeating part placement, 95 Replace
Index library, 84 multiple elements, 182 multiple objects, 116 objects on schematic, 116 part by description, 83 part by name, 81 part for editing, 188 part from symbol library, 84 parts, 8 selection area definition of, 336 selection rectangle, 116 Set Attribute Level dialog box, 242 Set Attribute Value dialog box, 11, 105 Set Up Block dialog box, 229, 248 setpoint definition of, 336 setting autosave interval, 58 border style, 50 default properties, 60 outline border, 50 package class priorities, 284 scale
Index editing, 2, 94, 188 elements of, 178 exporting, 174 global port, 102 hierarchical, 233 library, 42, 80, 173, 321 placing, 85 port, 30 primitive, 233 printing, 167 stopping placement, 85 wiring, 247 symbol aliases, 200 symbol attribute COMPONENT, 316 GATE, 316 GATETYPE, 316 MODEL, 316 PART, 317 PKGREF, 317 PKGTYPE, 317 REFDES, 318 SIMULATION- ONLY, 318 TEMPLATE, 318 symbol editor automatically starting, 152 closing, 152 creating annotation symbols, 134 exporting, 304 importing graphics, 181 part attrib
Index Enable Bias Voltage Display, 37 Get New Part, 82, 155 Insert Picture, 38, 133, 181 Marker Color, 36 More Info, 76 New File, 33, 79, 154 New Symbol, 155, 172 Open File, 33, 79, 154 Place Pins, 155, 180 Print, 33, 140 Redraw, 34, 39, 153, 155 Save File, 33, 154, 248 Select Part, 8, 35, 245 Show/Hide Currents on Selected Part(s), 37 Show/Hide Voltage on Selected Net(s), 37 Simulation, 36 Voltage/Level Marker, 36 Zoom Area, 34, 68, 154 Zoom In, 34, 68, 154 Zoom Out, 34, 69, 154 Zoom to Fit Page, 34, 70, 1
Index moving, 15 orthogonal, 109 rewiring segment, 105 selecting, 116 wire segment adding, 104 wiring symbols, 247 wizard symbol creation, 171 workspaces, 19 Z zoned border style, 53 Zoom Area button, 34, 68, 154 zoom factor, 142 Zoom In button, 34, 68, 154 Zoom Out button, 34, 69, 154 zoom parameters setting, 69 Zoom to Fit Page button, 34, 70, 154 352
