Orcad Capture User's Guide PSpice Or CAD

PSpice_CaptureGuideOrCAD

User Manual:

Open the PDF directly: View PDF PDF.
Page Count: 374 [warning: Documents this large are best viewed by clicking the View PDF Link!]

Orcad® Capture
User’s Guide
capug.book Page 1 Tuesday, May 23, 2000 12:08 PM
Cadence PCB Systems Division
13221 SW 68th Parkway, Suite 200
Portland, OR 97223
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.
Affirma, Assura, Cierto, Envisia, Mercury Plus, Quickturn, Radium, Silicon Ensemble,
and SPECCTRAQuest are trademarks of Cadence Design Systems, Inc.
Alanza is a service mark of Cadence Design Systems, Inc.
All other brand and product names mentioned herein are used for identification
purposes only and are registered trademarks, trademarks, or service marks of their
respective holders.
60-30-611
Second edition 31 May 2000
Cadence PCB Systems Division (PSD) offices
PSD main office (Portland) (503) 671-9500
PSD Irvine office (949) 788-6080
PSD Japan office 81-45-682-5770
PSD UK office 44-1256-381-400
PSD customer support (877) 237-4911
PSD web site www.orcad.com
PSD customer support web page www.orcad.com/technical/technical.asp
PSD customer support email form www.orcad.com/technical/email_support.asp
capug.book Page 2 Tuesday, May 23, 2000 12:08 PM
Contents
Contents iii
Before you begin xvii
Welcome . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xvii
How to use this guide . . . . . . . . . . . . . . . . . . . . . . . . . . . . xviii
Symbols and conventions . . . . . . . . . . . . . . . . . . . . . . . xviii
Related documentation . . . . . . . . . . . . . . . . . . . . . . . . . . xix
Part One Capture basics
Getting started 3Chapter 1 Starting Capture . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3
The Capture session frame . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
The Capture work environment 5Chapter 2 The project manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
Project manager folders . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
Project manager tabs—File and Hierarchy . . . . . . . . . . . . . . . . 9
Single view . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
Flat and hierarchical designs . . . . . . . . . . . . . . . . . . . . . . . . 10
Project manager pop-up menus . . . . . . . . . . . . . . . . . . . . . . 10
The schematic page editor . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
The part editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
The programmer’s editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
The session log . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
The toolbar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Displaying or hiding the toolbar . . . . . . . . . . . . . . . . . . . . . . 18
The tool palettes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
The schematic page editor tool palette . . . . . . . . . . . . . . . . . . 19
The part editor tool palette . . . . . . . . . . . . . . . . . . . . . . . . . 22
capug.book Page iii Tuesday, May 23, 2000 12:08 PM
Contents
iv
Displaying or hiding a tool palette . . . . . . . . . . . . . . . . . . . . 24
The status bar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
Left field . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
Center field . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
Right field . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
Displaying or hiding the status bar . . . . . . . . . . . . . . . . . . . 26
Selecting and deselecting objects . . . . . . . . . . . . . . . . . . . . . . . 27
Grouping objects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29
Editing properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30
Instance and occurrence properties . . . . . . . . . . . . . . . . . . . 31
Instance properties . . . . . . . . . . . . . . . . . . . . . . . . . . 31
Occurrence properties . . . . . . . . . . . . . . . . . . . . . . . . . 31
The Browse spreadsheet editor . . . . . . . . . . . . . . . . . . . . . . 32
The property editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
The property editor window . . . . . . . . . . . . . . . . . . . . . 36
The property editor Filter menu . . . . . . . . . . . . . . . . . . . 40
Using the property editor . . . . . . . . . . . . . . . . . . . . . . . 43
The Package Properties spreadsheet editor . . . . . . . . . . . . . . . 46
Moving and resizing graphic objects . . . . . . . . . . . . . . . . . . . . . 48
Undoing, redoing, and repeating an action . . . . . . . . . . . . . . . . . 49
Using the Accessories menu . . . . . . . . . . . . . . . . . . . . . . . . . 51
Starting a project 51Chapter 3 Creating new projects, designs, libraries, and VHDL files . . . . . . . . . 52
Opening existing projects, designs, libraries, and VHDL files . . . . . . 55
Working with files in a project . . . . . . . . . . . . . . . . . . . . . . . . 57
Saving projects, designs, and libraries . . . . . . . . . . . . . . . . . . . . 58
Closing a project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59
Archiving a project . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61
Setting up your project 63Chapter 4 Defining your preferences . . . . . . . . . . . . . . . . . . . . . . . . . . . 65
Defining colors/print options . . . . . . . . . . . . . . . . . . . . . . 66
Controlling the grid . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68
Setting pan and zoom . . . . . . . . . . . . . . . . . . . . . . . . . . . 69
Defining selection options . . . . . . . . . . . . . . . . . . . . . . . . 71
Setting miscellaneous options . . . . . . . . . . . . . . . . . . . . . . 73
Setting text editor options . . . . . . . . . . . . . . . . . . . . . . . . . 76
Setting up your project template . . . . . . . . . . . . . . . . . . . . . . . 78
Setting up fonts for new projects . . . . . . . . . . . . . . . . . . . . . 79
Defining title block information . . . . . . . . . . . . . . . . . . . . . 80
capug.book Page iv Tuesday, May 23, 2000 12:08 PM
Contents
v
Setting the schematic page size for new projects . . . . . . . . . . . . . 82
Defining the grid reference . . . . . . . . . . . . . . . . . . . . . . . . . 84
Defining the default hierarchy option for new projects . . . . . . . . . 86
Setting up compatibility with Orcads Schematic Design Tools (SDT) 87
Changing properties of existing projects . . . . . . . . . . . . . . . . . . . 88
Assigning fonts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89
Defining hierarchy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89
Using Capture with SDT . . . . . . . . . . . . . . . . . . . . . . . . . . 89
Viewing design information . . . . . . . . . . . . . . . . . . . . . . . . 90
Viewing and connecting to invisible power pins . . . . . . . . . . . . 91
Changing properties of existing schematic pages . . . . . . . . . . . . . . 92
Changing page size . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92
Setting up new grid references . . . . . . . . . . . . . . . . . . . . . . . 93
Viewing miscellaneous schematic page properties . . . . . . . . . . . 93
Printing and plotting 95Chapter 5 Printing or plotting schematic pages . . . . . . . . . . . . . . . . . . . . . 96
Printing or plotting parts or packages . . . . . . . . . . . . . . . . . . . . . 97
Printing the session log and text editor windows . . . . . . . . . . . . . . 98
Previewing printer or plotter output . . . . . . . . . . . . . . . . . . . . . 99
Scaling printer or plotter output . . . . . . . . . . . . . . . . . . . . . . . 100
Special considerations for plotting . . . . . . . . . . . . . . . . . . . . . . 101
Plotter pen colors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101
Part Two Creating designs
Design structure 105Chapter 6 Flat designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106
Hierarchical designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107
Simple hierarchical designs . . . . . . . . . . . . . . . . . . . . . . . 107
Complex hierarchies . . . . . . . . . . . . . . . . . . . . . . . . . . . 109
Connecting schematic folders and schematic pages . . . . . . . . . . . . 110
Hierarchical blocks . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110
Hierarchical ports . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111
Hierarchical pins . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111
Off-page connectors . . . . . . . . . . . . . . . . . . . . . . . . . . . . 112
An example: creating a simple hierarchy . . . . . . . . . . . . . . . . . . 113
Placing, editing, and connecting parts and symbols 115Chapter 7 Placing and editing parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 117
capug.book Page v Tuesday, May 23, 2000 12:08 PM
Contents
vi
Placing parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 118
Place Part dialog box . . . . . . . . . . . . . . . . . . . . . . . . . 121
Most Recently Used (MRU) part list . . . . . . . . . . . . . . . . . 124
Searching for parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125
Editing parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125
Placing and editing power and ground symbols . . . . . . . . . . . . . . 128
Placing power and ground symbols . . . . . . . . . . . . . . . . . . . 128
Place Power and Place Ground dialog boxes . . . . . . . . . . . . 130
Editing power and ground symbols . . . . . . . . . . . . . . . . . . . 131
Placing and editing no-connect symbols . . . . . . . . . . . . . . . . . . . 132
Placing no-connect symbols . . . . . . . . . . . . . . . . . . . . . . . 132
Editing no-connect symbols . . . . . . . . . . . . . . . . . . . . . . . 133
Placing and editing hierarchical blocks . . . . . . . . . . . . . . . . . . . 134
Placing hierarchical blocks . . . . . . . . . . . . . . . . . . . . . . . . 134
Place Hierarchical Block dialog box . . . . . . . . . . . . . . . . . 136
Editing hierarchical blocks . . . . . . . . . . . . . . . . . . . . . . . . 138
Placing and editing hierarchical ports and hierarchical pins . . . . . . . 139
Placing hierarchical ports . . . . . . . . . . . . . . . . . . . . . . . . . 139
Place Hierarchical Port dialog box . . . . . . . . . . . . . . . . . 140
Placing hierarchical pins . . . . . . . . . . . . . . . . . . . . . . . . . 141
Place Hierarchical Pin dialog box . . . . . . . . . . . . . . . . . . 143
Editing hierarchical ports and hierarchical pins . . . . . . . . . . . . 143
Placing and editing off-page connectors . . . . . . . . . . . . . . . . . . . 144
Placing off-page connectors . . . . . . . . . . . . . . . . . . . . . . . . 144
Place Off-Page Connector dialog box . . . . . . . . . . . . . . . . 146
Editing off-page connectors . . . . . . . . . . . . . . . . . . . . . . . . 147
Placing and connecting wires and buses . . . . . . . . . . . . . . . . . . . 148
Placing wires . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149
Editing wires . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150
Moving wires . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151
Placing buses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 152
Editing buses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153
Placing bus entries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153
Editing bus entries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154
Ripping a subset of signals off the bus . . . . . . . . . . . . . . . . . . 155
Adding and editing graphics and text 157Chapter 8 Drawing tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 158
Drawing lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159
Drawing rectangles and squares . . . . . . . . . . . . . . . . . . . . . . . 160
Drawing circles and ellipses . . . . . . . . . . . . . . . . . . . . . . . . . 161
capug.book Page vi Tuesday, May 23, 2000 12:08 PM
Contents
vii
Drawing arcs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162
Drawing polylines and polygons . . . . . . . . . . . . . . . . . . . . . . 163
Adding fill to an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164
Mirroring an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164
Rotating an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165
Moving an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165
Cutting an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165
Copying an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166
Pasting an object . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166
Deleting a selected object . . . . . . . . . . . . . . . . . . . . . . . . . . . 166
Placing a bitmap . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167
Placing text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168
The text bounding box . . . . . . . . . . . . . . . . . . . . . . . . . . 170
Deleting text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 170
Modifying text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 170
Finding text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 171
Replacing text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 172
Importing text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 172
Exporting text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 173
Character formatting . . . . . . . . . . . . . . . . . . . . . . . . . . . 173
About screen fonts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 174
Using macros 175Chapter 9 Recording a macro . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177
Playing a macro . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 178
Configuring a macro . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 179
Configure Macro dialog box . . . . . . . . . . . . . . . . . . . . . 180
Naming a macro . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 183
Assigning a shortcut key to a macro . . . . . . . . . . . . . . . . . . . . . 185
Sample macros . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186
Changing your view of a schematic page 187Chapter 10 Zooming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 188
Zooming to a specified scale . . . . . . . . . . . . . . . . . . . . . . . 189
Other viewing options . . . . . . . . . . . . . . . . . . . . . . . . . . 189
Moving to a new location . . . . . . . . . . . . . . . . . . . . . . . . . . . 192
Moving to an X, Y location . . . . . . . . . . . . . . . . . . . . . . . . 192
Go To dialog box, Location tab . . . . . . . . . . . . . . . . . . . 193
Jumping to a specific grid reference . . . . . . . . . . . . . . . . . . . 194
Go To dialog box, Grid Reference tab . . . . . . . . . . . . . . . . 194
Jumping to a marked location . . . . . . . . . . . . . . . . . . . . . . 195
capug.book Page vii Tuesday, May 23, 2000 12:08 PM
Contents
viii
Go To dialog box, Bookmark tab . . . . . . . . . . . . . . . . . . . 196
Displaying the grid and grid references . . . . . . . . . . . . . . . . . . . 197
Finding parts in a project . . . . . . . . . . . . . . . . . . . . . . . . . . . 198
Part Three Libraries and parts
About libraries and parts 201Chapter 11 Libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 202
Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 203
About part instances and part occurrences . . . . . . . . . . . . . . . 204
The design cache . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 205
Primitive and nonprimitive parts . . . . . . . . . . . . . . . . . . . . . . . 208
Creating and editing parts 209Chapter 12 Parts and packages: homogeneous or heterogeneous . . . . . . . . . . . 210
Creating a new part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 211
Defining a part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 211
New Part Properties dialog box . . . . . . . . . . . . . . . . . . . 214
Attaching a schematic folder to a part . . . . . . . . . . . . . . . . . . 216
Adding graphics, text, and IEEE symbols to a part . . . . . . . . . . 217
Placing pins on a part . . . . . . . . . . . . . . . . . . . . . . . . . . . 218
Place Pin dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . 220
Place Pin Array dialog box . . . . . . . . . . . . . . . . . . . . . . 225
About power and ground pins . . . . . . . . . . . . . . . . . . . . . . . . 227
Displaying invisible power pins . . . . . . . . . . . . . . . . . . . . . 228
Editing an existing part . . . . . . . . . . . . . . . . . . . . . . . . . . . . 229
Editing a part in a library . . . . . . . . . . . . . . . . . . . . . . . . . 229
Editing a part on a schematic page . . . . . . . . . . . . . . . . . . . . 230
Editing part properties . . . . . . . . . . . . . . . . . . . . . . . . . . 231
Default part properties . . . . . . . . . . . . . . . . . . . . . . . . 232
Viewing parts in a package . . . . . . . . . . . . . . . . . . . . . . . . . . 234
Editing parts in a package . . . . . . . . . . . . . . . . . . . . . . . . . . . 235
Editing part and package properties in the part editor . . . . . . . . . . 236
Viewing a parts convert . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239
Part Four Processing your design
About the processing tools 243Chapter 13 Tools overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 244
capug.book Page viii Tuesday, May 23, 2000 12:08 PM
Contents
ix
Updating instances and occurrences . . . . . . . . . . . . . . . . . . 246
Preparing to create a netlist 247Chapter 14 Annotating . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 247
Annotate dialog box . . . . . . . . . . . . . . . . . . . . . . . . . 249
Updating properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 251
Update Properties dialog box . . . . . . . . . . . . . . . . . . . . 253
Update file format . . . . . . . . . . . . . . . . . . . . . . . . . . . 255
Checking for design rules violations . . . . . . . . . . . . . . . . . . . . 256
Design Rules Check dialog box, Design Rules Check tab . . . . 259
Design Rules Check dialog box, ERC Matrix tab . . . . . . . . . 262
Sample Design Rules Check report . . . . . . . . . . . . . . . . . 263
Back annotating . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 266
Back Annotate dialog box . . . . . . . . . . . . . . . . . . . . . . 268
Swap file format . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269
Creating a netlist 271Chapter 15 Using the Create Netlist tool . . . . . . . . . . . . . . . . . . . . . . . . . 271
Netlist format files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 273
Netname resolution . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274
Creating reports 275Chapter 16 Creating a bill of materials . . . . . . . . . . . . . . . . . . . . . . . . . . 275
Bill of Materials dialog box . . . . . . . . . . . . . . . . . . . . . . 277
Include file format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 279
Creating a cross reference report . . . . . . . . . . . . . . . . . . . . . . . 280
Cross Reference Parts dialog box . . . . . . . . . . . . . . . . . . 281
Exporting and importing schematic data 283Chapter 17 Exporting and importing designs . . . . . . . . . . . . . . . . . . . . . . 283
Exporting designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284
Importing designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 285
Exporting and importing properties . . . . . . . . . . . . . . . . . . . . . 286
Exporting properties . . . . . . . . . . . . . . . . . . . . . . . . . . . 286
Property file format . . . . . . . . . . . . . . . . . . . . . . . . . . . . 288
Editing a property file . . . . . . . . . . . . . . . . . . . . . . . . . . . 288
Importing properties . . . . . . . . . . . . . . . . . . . . . . . . . . . 290
Generating a part 293Chapter 18 Using the Generate Part tool . . . . . . . . . . . . . . . . . . . . . . . . . 294
capug.book Page ix Tuesday, May 23, 2000 12:08 PM
Contents
x
Generate a new part . . . . . . . . . . . . . . . . . . . . . . . . . . . . 294
Update the pin numbers of an existing part . . . . . . . . . . . . . . 297
Using Capture with Orcad Layout 299Chapter 19 Preparing your Capture design for use with Layout . . . . . . . . . . . . 301
Creating a netlist for use in Layout . . . . . . . . . . . . . . . . . . . . . . 303
Loading a new netlist into Layout . . . . . . . . . . . . . . . . . . . . . . 304
Back annotating board information from Layout . . . . . . . . . . . . . . 306
Forward annotating schematic data to Layout . . . . . . . . . . . . . . . 307
Cross probing between Capture and Layout . . . . . . . . . . . . . . . . 308
Enabling intertool communication between Capture and Layout . . 308
Cross probing from Capture to Layout . . . . . . . . . . . . . . . . . 309
Cross probing from Layout to Capture . . . . . . . . . . . . . . . . . 310
General rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311
Using Capture with PSpice 313Chapter 20 Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 313
Specifying simulation model libraries . . . . . . . . . . . . . . . . . . . . 314
Creating a design for PSpice A/D simulation . . . . . . . . . . . . . . . . 315
Editing simulation models from Capture . . . . . . . . . . . . . . . . . . 316
Adding and defining stimulus . . . . . . . . . . . . . . . . . . . . . . . . 317
Placing stimulus sources . . . . . . . . . . . . . . . . . . . . . . . . . 317
Using the Stimulus Editor . . . . . . . . . . . . . . . . . . . . . . . . . 317
Setting up and running analyses . . . . . . . . . . . . . . . . . . . . . . . 318
Viewing results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319
Viewing results as you simulate . . . . . . . . . . . . . . . . . . . . . 319
Using markers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319
Configuring the display of simulation results . . . . . . . . . . . . . 320
Creating designs for PSpice simulation and board layout . . . . . . . . . 321
Handling unmodeled pins . . . . . . . . . . . . . . . . . . . . . . . . 322
Displaying bias point information . . . . . . . . . . . . . . . . . . . . . . 323
Displaying bias point values . . . . . . . . . . . . . . . . . . . . . . . 323
Glossary 325
Index 337
capug.book Page x Tuesday, May 23, 2000 12:08 PM
Figures
Figure 1 Captures session frame . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
Figure 2 New project manager window . . . . . . . . . . . . . . . . . . . . . . . . . 6
Figure 3 File tab . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
Figure 4 Hierarchy tab . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
Figure 5 Schematic page editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11
Figure 6 Part editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
Figure 7 Programmers editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
Figure 8 Session log . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
Figure 9 Captures toolbar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Figure 10 Schematic page editor tool palette . . . . . . . . . . . . . . . . . . . . . . . 19
Figure 11 Part editor tool palette . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22
Figure 12 The status bar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25
Figure 13 Browse spreadsheet editor . . . . . . . . . . . . . . . . . . . . . . . . . . . 32
Figure 14 Property editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36
Figure 15 Package Properties spreadsheet editor . . . . . . . . . . . . . . . . . . . . 46
Figure 16 Open project, design, and schematic page . . . . . . . . . . . . . . . . . . 55
Figure 17 Open library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56
Figure 18 Open VHDL file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56
Figure 19 Colors/Print tab of the Preferences dialog box . . . . . . . . . . . . . . . . 66
Figure 20 Grid Display tab of the Preferences dialog box . . . . . . . . . . . . . . . . 68
Figure 21 Pan and Zoom tab of the Preferences dialog box . . . . . . . . . . . . . . . 69
Figure 22 Select tab of the Preferences dialog box . . . . . . . . . . . . . . . . . . . . 71
Figure 23 Miscellaneous tab of the Preferences dialog box . . . . . . . . . . . . . . . 73
Figure 24 Text Editor tab of the Preferences dialog box . . . . . . . . . . . . . . . . . 76
Figure 25 Fonts tab of the Design Template dialog box . . . . . . . . . . . . . . . . . 79
Figure 26 Title Block tab of the Design Template dialog box . . . . . . . . . . . . . . 80
Figure 27 Title block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81
Figure 28 Page Size tab of the Design Template dialog box . . . . . . . . . . . . . . 82
Figure 29 Grid Reference tab of the Design Template dialog box . . . . . . . . . . . 84
Figure 30 Hierarchy tab of the Design Template dialog box . . . . . . . . . . . . . . 86
Figure 31 SDT Compatibility tab of the Design Template dialog box . . . . . . . . . 87
Figure 32 Miscellaneous tab of the Design Properties dialog box . . . . . . . . . . . 90
capug.book Page xi Tuesday, May 23, 2000 12:08 PM
Figures
xii
Figure 33 Miscellaneous tab of the Schematic Page Properties dialog box . . . . . 93
Figure 34 An abstract representation of a simple hierarchy. . . . . . . . . . . . . . 107
Figure 35 A simple hierarchical design, as seen in the project manager . . . . . . . 108
Figure 36 An abstract representation of a complex hierarchy . . . . . . . . . . . . . 109
Figure 37 A complex hierarchical design, as seen in the project manager . . . . . . 109
Figure 38 Schematics before hierarchy . . . . . . . . . . . . . . . . . . . . . . . . . . 113
Figure 39 Schematics with hierarchy . . . . . . . . . . . . . . . . . . . . . . . . . . . 113
Figure 40 Schematics carrying a net . . . . . . . . . . . . . . . . . . . . . . . . . . . 114
Figure 41 Connectivity across pages in a schematic . . . . . . . . . . . . . . . . . . 114
Figure 42 Schematic with power and ground symbols . . . . . . . . . . . . . . . . 115
Figure 43 Part editor in package view . . . . . . . . . . . . . . . . . . . . . . . . . . 117
Figure 44 Part editor in part view . . . . . . . . . . . . . . . . . . . . . . . . . . . . 118
Figure 45 Place Part dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121
Figure 46 Property editor with filter set to Capture . . . . . . . . . . . . . . . . . . 126
Figure 47 Power and ground symbols in CAPSYM.OLB . . . . . . . . . . . . . . . 128
Figure 48 Place Power dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130
Figure 49 Hierarchical block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134
Figure 50 Place Hierarchical Block dialog box . . . . . . . . . . . . . . . . . . . . . 136
Figure 51 Hierarchical ports in CAPSYM.OLB . . . . . . . . . . . . . . . . . . . . . 139
Figure 52 Place Hierarchical Port dialog box . . . . . . . . . . . . . . . . . . . . . . 140
Figure 53 Place Hierarchical Pin dialog box . . . . . . . . . . . . . . . . . . . . . . . 143
Figure 54 Off-page connectors in CAPSYM.OLB . . . . . . . . . . . . . . . . . . . . 144
Figure 55 Place Off-Page Connector dialog box . . . . . . . . . . . . . . . . . . . . 146
Figure 56 Connectivity change warning . . . . . . . . . . . . . . . . . . . . . . . . . 151
Figure 57 Schematic page editor tool palette . . . . . . . . . . . . . . . . . . . . . . 158
Figure 58 Part editor tool palette . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 158
Figure 59 Configure Macro dialog box . . . . . . . . . . . . . . . . . . . . . . . . . 180
Figure 60 Location tab of the Go To dialog box . . . . . . . . . . . . . . . . . . . . . 193
Figure 61 Grid Reference tab of the Go To dialog box . . . . . . . . . . . . . . . . . 194
Figure 62 Bookmark tab of the Go To dialog box . . . . . . . . . . . . . . . . . . . . 196
Figure 63 Replace Cache dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 206
Figure 64 New Part Properties dialog box . . . . . . . . . . . . . . . . . . . . . . . . 214
Figure 65 Place Pin dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 220
Figure 66 Place Pin Array dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . 225
Figure 67 User Properties dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . 232
Figure 68 Part editor in Package View . . . . . . . . . . . . . . . . . . . . . . . . . . 234
Figure 69 Edit Part Properties dialog box . . . . . . . . . . . . . . . . . . . . . . . . 237
Figure 70 Before annotation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 248
Figure 71 After annotation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 248
Figure 72 Annotate dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 249
Figure 73 Update Properties dialog box . . . . . . . . . . . . . . . . . . . . . . . . . 253
Figure 74 Design Rules Check tab of the Design Rules Check dialog box . . . . . . 259
capug.book Page xii Tuesday, May 23, 2000 12:08 PM
Figures
xiii
Figure 75 ERC tab of the Design Rules Check dialog box . . . . . . . . . . . . . . . 262
Figure 76 Back Annotate dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 268
Figure 77 Create Netlist dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 272
Figure 78 Bill of Materials dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . 277
Figure 79 Cross Reference Parts dialog box . . . . . . . . . . . . . . . . . . . . . . 281
Figure 80 Export Design dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 284
Figure 81 Import Design dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 285
Figure 82 Export Properties dialog box . . . . . . . . . . . . . . . . . . . . . . . . . 287
Figure 83 Import Properties dialog box . . . . . . . . . . . . . . . . . . . . . . . . . 291
Figure 84 Generate Part dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 295
Figure 85 Generate Part dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 297
capug.book Page xiii Tuesday, May 23, 2000 12:08 PM
Figures
xiv
capug.book Page xiv Tuesday, May 23, 2000 12:08 PM
Tables
Table 1 Tools on the Capture toolbar . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Table 2 Tools on the schematic page editor tool palette . . . . . . . . . . . . . . . 20
Table 3 Tools on the part editor tool palette . . . . . . . . . . . . . . . . . . . . . . 22
Table 4 Captures macro subroutines . . . . . . . . . . . . . . . . . . . . . . . . . 183
Table 5 Valid shortcut keys . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186
Table 6 Pin shapes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 221
Table 7 Pin types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 222
Table 8 Capture tools overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . 245
Table 9 Updating instances or occurrences . . . . . . . . . . . . . . . . . . . . . 246
Table 10 Netlist format file types . . . . . . . . . . . . . . . . . . . . . . . . . . . . 273
Table 11 Action on part or pin properties . . . . . . . . . . . . . . . . . . . . . . . 290
Table 12 Cross probing from Capture to Layout . . . . . . . . . . . . . . . . . . . 309
Table 13 Cross probing from Layout to Capture . . . . . . . . . . . . . . . . . . . 310
capug.book Page xv Tuesday, May 23, 2000 12:08 PM
Tables May 22, 2000
xvi
capug.book Page xvi Tuesday, May 23, 2000 12:08 PM
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.
Whats more, Orcad family products are a suite of
applications built around an engineer's design flownot
just a collection of independently developed point tools.
Orcad Capture is just one element in our total solution
design flow.
Capture is a versatile design entry product you can use to
create schematics for analog or mixed signal designs,
printed circuit board layout designs, and programmable
logic designs. First, create your flat or hierarchical design
in the schematic page editor, then use Captures tools to
quickly annotate it and prepare it for the next stage of
development.
capug.book Page xvii Tuesday, May 23, 2000 12:08 PM
Before you begin
xviii
How to use this guide
This guide is designed so you can quickly find the
information you need to use Insert Product Name. To help
you learn and use Insert Product Name efficiently, this
manual is separated into the following sections:
Part 1, Capture basics, includes how to get started
with Capture; what you need to know about the
Capture windows, editors, session log, the toolbar and
tool palettes, and general Capture concepts; how to
start and set up a project; and printing and plotting.
Part 2, Creating designs, discusses design structure;
placing, editing, and connecting parts and symbols;
adding and editing graphics and text; using macros,
and changing your schematic page view.
Part 3, Libraries and parts, tells you about libraries and
parts, and how to create and edit parts.
Part 4, Processing your design, provides an overview
of the processing tools; creating a netlist and reports;
exporting and importing schematic data; generating a
part; and using Capture with Orcad Layout and
PSpice.
Symbols and conventions
Our printed documentation uses a few special symbols
and conventions.
Notation Examples Description
C+rPress C+r.Means to hold down the C key while
pressing r.
A, f, oFrom the File menu, choose Open (A, f,
o). Means that you have two options. You
can use the mouse to choose the Open
command from the File menu, or you
can press each of the keys in
parentheses in order: first A, then f,
then o.
capug.book Page xviii Tuesday, May 23, 2000 12:08 PM
How to use this guide
xix
Related documentation
In addition to this guide, you can find technical product
information in the online help, the online interactive
tutorial, online books, and our technical web site, as well
as in other books. The table below describes the types of
technical documentation provided with Insert Product
Name.
Monospace font In the Part Name text box, type PARAM.Text that you type is shown in
monospace font. In the example, you
type the characters P, A, R, A, and
M.
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.
This documentation component . . . Provides this . . .
This guide
Orcad Capture User’s Guide A comprehensive guide for understanding and using the
features available in Insert Product Name.
capug.book Page xix Tuesday, May 23, 2000 12:08 PM
Before you begin
xx
Online help Comprehensive information for understanding and using
the features available in Insert Product Name.
You can access help from the Help menu in Insert Product
Name by choosing the Help button in a dialog box, or by
pressing 1. Topics include:
Explanations and instructions for common tasks.
Descriptions of menu commands, dialog boxes, tools on
the toolbar and tool palettes, and the status bar.
Error messages and glossary terms.
Reference information.
Product support information.
You can get context-sensitive help for a error message by
placing your cursor in the error message line in the session
log and pressing 1.
Online interactive tutorial A series of self-paced interactive lessons. You can practice
what youve learned by going through the tutorials
specially designed exercises that interact directly with
Insert Product Name. You can start the tutorial by choosing
Learning Insert Product Name from the Help menu.
Online Orcad Capture Users Guide An online, searchable version of this guide, available when
choosing Online Manuals from the Orcad family program
group (on the Start menu).
Online Insert Product Name quick reference Concise descriptions of the commands, shortcuts, and tools
available in Insert Product Name, available when choosing
Online Manuals from the Orcad family program group (on
the Start menu).
This documentation component . . . Provides this . . .
capug.book Page xx Tuesday, May 23, 2000 12:08 PM
How to use this guide
xxi
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. It also contains answers to
frequently asked questions.
The Knowledge Exchange, which enables you to share
information and ideas with other users and with our
technical experts in a real-time online forum. You can
submit issues or questions for open discussion, search
the Knowledge Exchange for information, or send email
to another participant for one-on-one communication. A
list of new postings will appear each time you visit the
Knowledge Exchange, providing you with a quick
update of whats been discussed since your last visit.
The Technical Library, which contains online customer
support information that you can search through by
category or product. You can find product manuals,
product literature, technical notes, articles, samples,
books, and other technical information. Additionally,
technical information can be obtained through
SourceLink, which is an online customer support
information service for users of Cadence software other
than Capture, Component Information System (CIS),
Express, Layout, or PSpice.
The Support Connection, which allows you to choose to
either view and update existing incidents, or create new
incidents. The information is delivered directly to us via
our internal database. This service is only available to
customers with current maintenance or Extended
Support Options (ESOs) in the United States and
Canada.
The Live Connection, which enables you to open access
to your computer to a Customer Support person, who
can then view your actions on your computer monitor
as you demonstrate the problem youre having. Live
Connections two-way transmission can also let you
view the actions on the Customer Support persons
computer monitor, as he or she demonstrates a method
or procedure to help you solve your problem. To
participate in Live Connection, you need to contact a
Customer Support person, in order to obtain a support
number to grant you access to the Live Connection site,
and to set up a time to meet online using Live
Connection.
This documentation component . . . Provides this . . .
capug.book Page xxi Tuesday, May 23, 2000 12:08 PM
Before you begin
xxii
capug.book Page xxii Tuesday, May 23, 2000 12:08 PM
Part One
Capture basics
Chapter 1, Getting started, describes how to start Capture.
Chapter 2, The Capture work environment, orients you to
Capture windows, the toolbar and tool palettes, and
general Capture concepts such as selecting and editing
objects, and undoing and repeating actions.
Chapter 3, Starting a project, describes the different types of
designs that Capture supports: flat, simple hierarchical,
and complex hierarchical. It introduces the electrical
objects used to create these types of designs, and provides
an example of how to create a simple hierarchy.
Chapter 4, Setting up your project, shows how to open a
design and navigate the schematics and schematic pages
in a design, or a portion of a design, such as an individual
schematic page.
Chapter 5, Printing and plotting, explains how to print or
plot schematic pages, parts, packages, the session log, or
text, and how to scale and preview printer or plotter
output.
capug.book Page 1 Tuesday, May 23, 2000 12:08 PM
capug.book Page 2 Tuesday, May 23, 2000 12:08 PM
Getting started
1
This chapter describes how to start Orcad Capture and
provides an overview of the Capture session frame.
Starting Capture
The Orcad Family installation process offers a default
location for Capture and adds Orcad Family Release to
the Programs menu (available from the Start button).
To start Capture
1From the Start menu, point to Programs and choose
Orcad Family Release.
2From the Orcad Family Release menu item, choose
Capture.
capug.book Page 3 Tuesday, May 23, 2000 12:08 PM
Chapter 1 Getting started
4
The Capture session frame
Once you start Capture, you see the Capture session frame.
You do all your schematic design and processing within
this window.
Figure 1 Captures session frame
The minimized Session Log icon in the lower left portion
of the Capture session frame is the session log. The session
log provides information about everything you have done
in the current Capture session. Detailed information about
this windowand the other windows in Captureis
given in Chapter 2, The Capture work environment.
In Capture, each design that you open is in a separate
project manager window. If you need to work
simultaneously with several designs, you can open them
all, and each will have its own project manager window.
Depending on which type of window you have active (an
active window is one whose title bar is highlighted),
certain buttons on the toolbar and certain items on the
menus may be unavailable, since you perform tasks and
use tools based upon the type of window that is active.
Also, the menus and menu choices vary, depending on
which type of window is active. The available menus and
menu choices also vary depending upon the type of
project.
capug.book Page 4 Tuesday, May 23, 2000 12:08 PM
The Capture work
environment
2
This chapter describes the things you need to know to find
your way around in Capture. It shows the windows youll
see in Capture: the project manager, the schematic page
editor, the part editor, the text editor, and the session log.
It also introduces you to the toolbar, tool palettes, and
general Capture concepts such as selecting and editing
objects, editing properties, and undoing and repeating
actions.
capug.book Page 5 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
6
The project manager
You use the project manager to collect and organize all the
resources you need for your project. These resources
include schematic folders, schematic pages, part libraries,
parts, VHDL files, and output reports such as bills of
materials and netlists. Figure 2 shows a new project
manager window.
A project doesnt actually contain all the resources. It
merely points to the various files that the project uses.
For this reason, be sure you dont move or delete any files
referenced by a project. If you do, the project wont be able
to find them.
The project file is saved with an .OPJ file extension. It is an
ASCII file, and can be viewed in any text editor.
Project manager folders
The project manager provides a graphical display of a
project’s resources by grouping them into appropriate
folders, as described below.
Shown underneath the Design Resources folder is the
design folder with the designs schematic folders and
schematic pages, and a Design Cache folder that
shows all the parts used on the schematic pages.
Capture automatically adds any schematic folders or
schematic pages that you create to the design folder.
(In Figure 2, the design folder is named
DESIGN3.DSN.) You can add other files or
information using the Project command on the Edit
menu. For example, you can add an existing VHDL
file to the design folder and later attach the models
within that VHDL file to hierarchical blocks on a
schematic page.
Figure 2 New project manager window
For information about hierarchical designs,
see Chapter 6, Design structure.
capug.book Page 6 Tuesday, May 23, 2000 12:08 PM
The project manager
7
The Library folder (in the Design Resources folder)
shows the schematic part library files youve added to
the project using the Project command on the Edit
menu.
The Outputs folder shows the output of Captures
processing tools. Generally, these files include bill of
materials reports and technology-specific netlists.
Capture adds files to this folder when each is created.
Each project may have only one design, but may have
multiple libraries. The design may consist of any number
of schematics or VHDL models, but it must have a single
root module. The root module is defined as the top level of
the design. That is, all other modules in the design are
referenced within the root module.
Within the project manager, you can expand or collapse
the structure you see by double-clicking on a folder, or by
clicking on the plus sign or minus sign to the left of a
folder. A plus sign indicates that the folder has contents
that are not currently visible; a minus sign indicates that
the folder is open and its contents are visible, listed below
the folder. It appears as a schematic folder with a slash on
it in a design file, or as a page in a VHDL file.
Each project you open has its own project manager
window. You can move or copy folders or files between
projects by dragging them from one project manager
window to another (as well as to and from Windows
Explorer). To copy rather than move items, press and hold
the C key while you drag them. If you close a project
manager window, you close the project.
In the project managers File tab, double-clicking on a
schematic folder expands it and displays icons for each
schematic page within the schematic folder. Then, if you
double-click on a schematic page icon, the schematic page
opens in a schematic page editor. Or, if the page is already
open, its window becomes active.
T
ip The root module for a design has a
backslash in its folder icon, as shown in
Figure 2 on page 2-6.
Note If a schematic page is open, you
cannot drag its icon to a different location.
capug.book Page 7 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
8
A design can consist of a single schematic page within a
single schematic folder, or a number of schematic pages
within a number of schematic folders. A schematic folder
contains schematic pages in a relationship similar to that
of a directory and the files it contains. Files are contained
in a directory; schematic pages are contained in a
schematic folder.
A schematic page provides a graphical description of the
electrical connectivity of a design. It is made up of parts,
wires, and other electrical symbols. A schematic page may
also contain borders, title blocks, text, and graphics.
Capture acts on any schematic folders or schematic pages
you have selected within an active project manager
window. For example, the Find and Browse commands on
the project managers Edit menu, the Print command on
the project managers File menu, and the various tools on
the Tools menu only apply to the selected schematic folder
or page.
Note T
h
e project manager is a
l
so use
d
to
manage libraries and the parts they
contain. This is covered in detail in
Chapter11, About libraries and parts.
capug.book Page 8 Tuesday, May 23, 2000 12:08 PM
The project manager
9
Project manager tabsFile and Hierarchy
The project manager provides two ways to display a
projects resources.
If you choose the File tab (shown in Figure 3), the project
manager displays all the projects folders, schematic
folders, and schematic pages. These are displayed in a
tree-like fashion. You can expand or collapse the tree by
clicking the plus sign in front of the icon. When that
branch of the tree is expanded, the plus sign change to a
minus sign.
If you choose the Hierarchy tab (shown in Figure 4), the
project manager displays the hierarchical relationship
among the projects schematic folders and schematic
pages.
For information about simple and complex hierarchical
designs, see Chapter 6, Design structure.
Single view
In Capture v7.2 and earlier versions, Capture uses logical
view and physical view to separate instance and
occurrence information. In Capture Release 9 and later,
both instances and occurrences are together in a single
view. The project manager shows all occurrences in the
Hierarchy tab.
Capture v7.2 and earlier require you to change view
before creating a netlist for use with Orcad Layout. In
Capture Release 9 and later, the netlist tool provides an
option to use either the instance properties or the
occurrence properties for creating a netlist.
Figure 3 File tab
Figure 4 Hierarchy tab
capug.book Page 9 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
10
Flat and hierarchical designs
In Capture, you can organize your schematics into flat or
heretical structures and interface to downstream EDA
products using either flat (popular for PCB layout) or
hierarchical (popular for synthesis and simulation)
netlists. The schematic system also supports reuse of
schematics within a hierarchy so you only need to draw a
schematic once, then instance it in multiple places for a
variety of applications. This guide uses the following
nomenclature to describe the parts and part properties of
these reused schematics:
Simple hierarchy. A hierarchical schematic design with no
reuse.
Complex hierarchy. A hierarchical schematic design with
reuse.
Part instance properties. The properties of any part that
has been placed in a schematic.
Part occurrence properties. The properties of a part that
make it unique from others in reused schematics.
Required to create a flat netlist with Capture.
Project manager pop-up menus
Several pop-up menus are available in the project
manager window. Pop-up menus are available by clicking
the right mouse button. You can use the commands on
these pop-up menus to open a file or schematic page, or
edit and view the properties of the currently selected item.
capug.book Page 10 Tuesday, May 23, 2000 12:08 PM
The schematic page editor
11
The schematic page editor
In the schematic page editor, you can display and edit
schematic pages. You can place parts, wires, buses, and
draw graphics. The schematic page editor has a tool
palette that you can use to draw and place everything you
need to create a schematic page. You can print from within
the schematic page editor, or from the project manager
window.
Figure 5 Schematic page editor
capug.book Page 11 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
12
The part editor
Create and edit parts using the part editor.
Figure 6 Part editor
From the View menu of the part editor, you can choose
Part or Package. In Part view you can:
Create and edit parts and symbols, then store them in
new or existing libraries.
Create and edit power and ground symbols, off-page
connector symbols, and title blocks.
Use the tool palettes electrical tools to place pins on
parts, and its drawing tools to draw parts and
symbols.
Package view shows the entire package. A package is a
physical part that contains more than one logical part. You
can edit the properties of the entire package, such as part
reference, prefix, part alias, and so on. You cannot edit
individual parts in this view, but you can select individual
parts to edit by double-clicking on them.
The part editor is very similar to the symbol editor. The
main difference between the two is the symbol editors
lack of Pin and Pin Array tool palette buttons.
For more information, see The part
editor tool palette on page 2-22.
See Chapter 11, About libraries
and parts for complete definitions of
parts and packages. See Chapter 12,
Creating and editing parts for a
complete description of the part editor.
capug.book Page 12 Tuesday, May 23, 2000 12:08 PM
The programmer’s editor
13
The programmer’s editor
Use the programmers editor to create or view VHDL files
or other text files within Capture. VHDL keywords and
comments are displayed in the colors you specify. (From
the Options menu, choose Preferences and select the Text
Editor tab.)
Figure 7 Programmers editor
To create a new VHDL file in the programmers editor
1From the File menu, point to New, then choose VHDL
File. A blank VHDL file appears in the text editor.
To open a VHDL file in the programmers editor
1From the File menu, point to Open, then choose VHDL
File. The Open VHDL File dialog box appears.
2Select a file, then click OK.
Or
1In the project manager, select a VHDL file.
2Click the right mouse button, and choose Edit from the
pop-up menu.
N
ote
D
esigns an
d
parts o
f
d
esigns can
b
e
VHDL-based instead of schematic-based.
capug.book Page 13 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
14
The session log
The session log lists the events that have occurred during
the current Capture session, including messages resulting
from using Captures tools. To display context-sensitive
help for an error message, put the cursor in the error
message line in the session log and press 1.
The ruler along the top appears in either inches or
millimeters, depending on which measurement system
(U.S. or Metric) you have selected in the Windows Control
Panel. You can add tab settings to the ruler by clicking in
the ruler bar and dragging the tabs to different positions,
or remove them by dragging them down into the session
log window. Capture saves your tab settings so that they
reappear each time you start Capture.
Figure 8 Session log
You can search for information in the session log using the
Find command on the Edit menu. You can also save the
contents of the session log to a file, which is useful when
working with Orcads customer support staff to solve
technical problems. The default filename is SESSION.TXT.
T
ip
Y
ou can c
l
ear t
h
e session
l
og
b
y
choosing the Clear Session Log command,
or by pressing C+ X.
capug.book Page 14 Tuesday, May 23, 2000 12:08 PM
The session log
15
To display the session log
1Click on the session logs maximize button, or choose
Session Log from the Window menu.
To minimize the session log
1Click the minimize button on the title bar.
To copy session log text to the Clipboard
1Select the session log window to make it active.
2Select the text and choose Copy from the Edit menu.
To print the session log
1Select the session log window to make it active.
2From the File menu, choose the Print command.
To use Find in the session log
1Select the session log window to make it active.
2From the Edit menu, choose the Find command. The
Find dialog box appears.
3Enter the word or words that you want to find.
4Click Find Next.
To save the session log to a text file
1Select the session log window to make it active.
2From the File menu, choose the Save As command.
The Save As dialog box appears.
3Enter a file name in the File name text box. By default,
the session log is saved to SESSION.TXT in the current
directory. If necessary, specify a new location for the
file.
4Click Save. The session log text is saved to the file.
capug.book Page 15 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
16
The toolbar
Captures toolbar is dockable (that is, you can select an area
between buttons and drag the toolbar to a new location)
and resizable. By choosing a tool button, you can quickly
perform a task. If a tool button is dimmed, you cant
perform that task in the current situation.
Figure 9 Captures toolbar
Some of the tools operate only on what you have selected,
while others give you a choice of either operating on what
is selected or expanding the scope to the entire project.
Table 1 summarizes the tools on the toolbar. The tasks that
these tools perform are described throughout this manual.
Table 1 Tools on the Capture toolbar
Tool Name Description
New Create a new document based on the active document. Similar to the
New command on the File menu. For more information, see Creating
new projects, designs, libraries, and VHDL files on page 3-52.
Open Open an existing project or library. Similar to the Open command on
the File menu. For more information, see Opening existing projects,
designs, libraries, and VHDL files on page 3-55.
Save Save the active document, schematic, or part. Equivalent to the Save
command on the File menu. For more information, see Saving projects,
designs, and libraries on page 3-58.
Print Print the selected pages in the schematic folder, or the active schematic
page or part. Equivalent to the Print command on the File menu. For
more information, see Chapter 5, Printing and plotting.
Cut Remove the selected object and place it on the Clipboard. Equivalent to
the Cut command on the Edit menu.
Copy Copy the selected object to the Clipboard. Equivalent to the Copy
command on the Edit menu.
N
ote
Th
e too
lb
ar is a
l
ways
d
oc
k
e
d
on t
h
e
top edge of the session frame the first time
y
ou open a project in a new session frame
of Capture. The position of the tool palette
is not saved.
capug.book Page 16 Tuesday, May 23, 2000 12:08 PM
The toolbar
17
Paste Paste the contents of the Clipboard at the cursor. Equivalent to the
Paste command on the Edit menu.
Undo Undo the last command performed, if possible. Equivalent to the Undo
command on the Edit menu.
Redo Redo the last command performed, if possible. Equivalent to the Redo
command on the Edit menu.
MRU Place a part or symbol from the list of most recently used parts and
symbols. For more information, see To place a part using the Most
Recently Used (MRU) List on page 7-120.
Zoom In Zoom in to see a closer, enlarged view. Equivalent to choosing Zoom
and In from the View menu. For more information, see To zoom in on
page 10-188.
Zoom Out Zoom out to see more of your document. Equivalent to choosing Zoom
and Out from the View menu. For more information, see To zoom out
on page 10-188.
Zoom Area Specify an area of the schematic page or part to enlarge to fill the entire
window. Equivalent to choosing Zoom and Area from the View menu.
For more information, see To view a selected area on page 10-189.
Zoom All View the entire document. Equivalent to choosing Zoom and All from
the View menu. For more information, see To view the entire page or
part on page 10-191.
Annotate Assign part references to parts on the selected schematic pages.
Equivalent to the Annotate command on the Tools menu. For more
information, see Annotating on page 14-247.
Back Annotate Back annotate the selected schematic pages. Equivalent to the Back
Annotate command on the Tools menu. For more information, see
Back annotating on page 14-266.
Design Rules
Check Check for design rules violations on the selected schematic pages.
Equivalent to the Design Rules Check command on the Tools menu.
For more information, see Checking for design rules violations on
page 14-256.
Create Netlist Create a netlist for the selected schematic pages. Equivalent to the
Create Netlist command on the Tools menu. For more information, see
Using the Create Netlist tool on page 15-271.
Table 1 Tools on the Capture toolbar (continued)
capug.book Page 17 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
18
Displaying or hiding the toolbar
You can hide the toolbar, then display it again when you
need it.
To display or hide the toolbar
1From the schematic page editors View menu, choose
Toolbar.
or
From the part editors View menu, choose Toolbar.
Cross Reference Create a cross reference report for the selected schematic pages.
Equivalent to the Cross Reference command on the Tools menu. For
more information, see Creating a cross reference report on
page 16-280.
Bill of Materials Create a bill of materials report for the selected schematic pages.
Equivalent to the Bill of Materials command on the Tools menu. For
more information, see Creating a bill of materials on page 16-275.
Snap-to-Grid Toggle schematic page and part editing to either on or off grid.
Project Manager Display the project manager window for the active document,
providing an overview of project contents. Equivalent to choosing a
project manager window by number from the Window menu.
Help Topics Open online help. Equivalent to the Help Topics command on the
Help menu.
Table 1 Tools on the Capture toolbar (continued)
capug.book Page 18 Tuesday, May 23, 2000 12:08 PM
The tool palettes
19
The tool palettes
Capture has two tool palettes: one for the schematic page
editor and one for the part editor. Both tool palettes are
dockable (that is, you can click on an area between buttons
and drag a tool palette to a new location) and resizable.
While the drawing tools on the two tool palettes are
identical, each tool palette has different electrical tools.
After you choose a tool (and, in the case of some tools,
after you respond to the tools dialog box), click the right
mouse button to display a context-sensitive pop-up menu.
The schematic page editor tool palette
The first group of tools on the tool palette is electrical
tools, used to place electrical connectivity objects. The
second group is drawing tools, used to create graphical
objects without electrical connectivity.
Figure 10 Schematic page editor tool palette
Table 2 describes the tools on the schematic page editor
tool palette.
Note The tool palette is always docked on
the right edge of the session frame the first
time you open a schematic page or part in
a new session of Capture. The position of
the tool palette is not saved.
For information on using the electrical
tools, see Chapter 7, Placing,
editing, and connecting parts and
symbols. For information on how to use
the drawing tools, see Chapter 8,
Adding and editing graphics and
capug.book Page 19 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
20
Table 2 Tools on the schematic page editor tool palette
Tool Name Description
Select Select objects. This is the normal mode.
Part Select parts from a library for placement.
Equivalent to the Part command on the Place
menu. For more information, see Placing parts on
page 7-118.
Wire Draw wires. Press and hold S to draw
non-orthogonal (not a multiple of 90°) wires.
Equivalent to the Wire command on the Place
menu. For more information, see Placing wires on
page 7-149.
Net Alias Place aliases on wires and buses. Equivalent to the
Net Alias command on the Place menu. For more
information, see Placing buses on page 7-152.
Bus Draw buses. Press S to draw
non-orthogonal segments. Equivalent to the Bus
command on the Place menu. For more
information, see Placing buses on page 7-152.
Junction Place junctions. Equivalent to the Junction
command on the Place menu.
Bus Entry Draw bus entries. Equivalent to the Bus Entry
command on the Place menu. For more
information, see Placing bus entries on
page 7-153.
Power Place power symbols. Equivalent to the Power
command on the Place menu. For more
information, see Placing power and ground
symbols on page 7-128.
Ground Place ground symbols. Equivalent to the Ground
command on the Place menu. For more
information, see Placing power and ground
symbols on page 7-128.
capug.book Page 20 Tuesday, May 23, 2000 12:08 PM
The tool palettes
21
Hierarchical
Block Place hierarchical blocks. Equivalent to the
Hierarchical Block command on the Place menu.
For more information, see Placing hierarchical
blocks on page 7-134.
Hierarchical
Port Place hierarchical ports on schematic pages.
Equivalent to the Hierarchical Port command on
the Place menu. For more information, see Placing
hierarchical ports on page 7-139.
Hierarchical
Pin Place hierarchical pins in hierarchical blocks.
Equivalent to the Hierarchical Pin command on
the Place menu. For more information, see Placing
hierarchical pins on page 7-141.
Off-Page
Connector Place off-page connectors. Equivalent to the
Off-Page Connector command on the Place menu.
For more information, see Placing off-page
connectors on page 7-144.
No Connect Place no-connect symbols on pins. Equivalent to
the No Connect command on the Place menu. See
Placing and editing no-connect symbols on
page 7-132.
Line Draw lines. Equivalent to the Line command on
the Place menu. For more information, see
Drawing lines on page 8-159.
Polyline Draw polylines. Press and hold S to draw
non-orthogonal polylines. Equivalent to the
Polyline command on the Place menu. For more
information, see Drawing polylines and polygons
on page 8-163.
Rectangle Draw rectangles. Holding S constrains to a
square. Equivalent to the Rectangle command on
the Place menu. For more information, see
Drawing rectangles and squares on page 8-160.
Ellipse Draw ellipses. Holding S constrains shape
to a circle. Equivalent to the Ellipse command on
the Place menu. For more information, see
Drawing circles and ellipses on page 8-161.
Table 2 Tools on the schematic page editor tool palette (continued)
capug.book Page 21 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
22
The part editor tool palette
The first group of tools on the part editor tool palette are
electrical tools, used to place pins and IEEE symbols. The
second group of tools are drawing tools, used to create
graphical objects without electrical connectivity.
Figure 11 Part editor tool palette
Table 3 describes the tools unique to the part editor tool
palette. The drawing tools are described in the previous
section, The schematic page editor tool palette on page 2-19.
Arc Draw arcs. Equivalent to the Arc command on the
Place menu. For more information, see Drawing
arcs on page 8-162.
Text Place text. Equivalent to the Text command on the
Place menu. For more information, see Placing
text on page 8-168.
Table 3 Tools on the part editor tool palette
Tool Name Description
IEEE
Symbol Place IEEE symbols on a part. Equivalent to the
IEEE Symbol command on the Place menu. For
more information, see Adding graphics, text, and
IEEE symbols to a part on page 12-217.
Table 2 Tools on the schematic page editor tool palette (continued)
For information on how to use the electrical
tools, see Chapter 12, Creating
and editing parts. For information on
how to use the drawing tools, see
Chapter 8, Adding and editing
capug.book Page 22 Tuesday, May 23, 2000 12:08 PM
The tool palettes
23
Pin Place pins on a part. Equivalent to the Pin
command on the Place menu. For more
information, see Placing pins on a part on
page 12-218.
Pin Array Place multiple pins on a part. Equivalent to the
Pin Array command on the Place menu. For more
information, see Placing pins on a part on
page 12-218.
Table 3 Tools on the part editor tool palette (continued)
capug.book Page 23 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
24
Displaying or hiding a tool palette
Like the toolbar, you can hide a tool palette, then display
it again when you need it.
To display or hide a tool palette
1From the schematic page editors View menu, choose
Tool Palette.
or
From the part editors View menu, choose Tool
Palette.
capug.book Page 24 Tuesday, May 23, 2000 12:08 PM
The status bar
25
The status bar
The status bar, located at the bottom of the Capture
session frame, reports on current actions, number of items
selected, zoom scale, and pointer location.
Figure 12 The status bar
Left field
The left field displays descriptions of selected tools or
menu items, prompts, or the current status.
Center field
The center field displays the number of items selected in
the schematic page editor or part editor.
Right field
The right field displays the current scale and pointer
location (such as: Scale=50% X=10.0 Y=5.0). The location
in the schematic page editor is measured in either inches
or millimeters, depending on the Units settings in the
Schematic Page Properties dialog box (Page Size tab). The
pointer location in the part editor is measured in grid
units.
N
ote
Wh
en a sess
i
on
l
og or a pro
j
ect
manager window is active, the center field
of the status bar doesn’t display.
capug.book Page 25 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
26
Displaying or hiding the status bar
You can hide the status bar, then display it again when
you need it.
To display or hide the status bar
1From the schematic page editors View menu, choose
Status Bar.
or
From the part editors View menu, choose Status Bar.
capug.book Page 26 Tuesday, May 23, 2000 12:08 PM
Selecting and deselecting objects
27
Selecting and deselecting objects
Once you select an object, you can perform operations on
it, including moving, copying, cutting, mirroring,
rotating, resizing, or editing. You can also select multiple
objects and edit them, or group them into a single object.
Grouping objects maintains the relationship among them
while you move them to another location.
This section describes different ways to select individual
objects and groups of objects in both the schematic page
editor and the part editor.
To select an object
1Position the pointer on the object and click the left
mouse button. The object displays in the selection
color.
To reset the selection color
1From the Options menu, choose Preferences, then
select the Colors tab.
2Click the left mouse button on the Selection color.
3Click to select a color from the Selection Color
window, then click OK. Click OK again to dismiss the
Preferences dialog box.
To select multiple objects
1For each object to select, position the pointer on the
object and hold C while you click the left mouse
button. Every object in the selection set displays in the
selection color.
To deselect objects
1Click on the schematic page away from any objects.
Selected objects become deselected. Keep in mind that
a part occupies a rectangular area encompassing all its
graphics. This means that a part may occupy a larger
area than is initially apparent.
Note You can edit the properties of a
g
roup of objects using the property editor.
See The property editor on page 34.
T
ip To select a part, click within the part
itself. To select a graphical object, zoom in
and click on an outside edge of the object.
capug.book Page 27 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
28
To select all objects in an area
1From the tool palette, choose the selection tool.
2Click on an area away from any objects or parts to
deselect any items that may be selected.
3Move the pointer to one corner of the area to select.
Press and hold the left mouse button while you drag
the mouse to the opposite corner, then release the left
mouse button. Every object in the selection set appears
in the selection color.
To include or exclude objects intersected by your selection
rectangle
1From the Options menu, choose Preferences.
2On the Select tab, select one of the Area Select options.
You can choose Intersecting to include items that are
not fully enclosed by your selection rectangle, or
choose Fully enclosed to exclude items that were not
entirely selected.
To select all objects on a schematic page or part
1From the Edit menu, choose Select All. All objects
appear in the selection color.
To select an object from a set of objects stacked atop one another
1Position the pointer over the stack of objects.
2Press F while you click the left mouse button. This
cycles through the objects in the stack.
To remove one object from a selection set
1Place the pointer over the object, press C, and click
the left mouse button.
N
ote
A
se
l
ect
i
on set
b
e
h
aves as
if
i
t
i
s one
object, so you can move, copy, cut, delete,
mirror, or rotate the entire set. Be aware,
however, that the Select All command also
selects the title block on the schematic
page. If you copy or move the selection set,
y
ou could create a duplicate title block, or
inadvertently move the title block off the
schematic page.
capug.book Page 28 Tuesday, May 23, 2000 12:08 PM
Selecting and deselecting objects
29
Grouping objects
Use the Group command on the Edit menu to group
multiple objects into one selectable object. This is a
convenient way to maintain the relationship among
several objects while moving them to another location.
You can nest groups, meaning a group can contain other
groups as well as objects.
The Group command is only available when multiple
objects are selected. Objects remain grouped until you
ungroup them or close the schematic page or part that
contains them.
To group multiple selected objects
1Select the objects you want to group. (See Selecting and
deselecting objects on page 2-26 for more information).
2From the Edit menu, choose Group. You can move the
objects as a group.
3When have finished working with the objects as a
group, you can ungroup them. From the Edit menu,
choose Ungroup.
Caution The Group command will not be
available if your selection includes a net
alias (a property). After block selecting the
objects you want to group, deselect the
included net aliases by holding the C
key and clicking on each object.
capug.book Page 29 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
30
Editing properties
In a Capture schematic design, each object has properties
that define their characteristics. These objects include:
Parts (including hierarchical blocks)
Nets (including constituent nets within buses)
Pins
Globals
Aliases
Hierarchical ports
Off-page connectors
DRC markers
Bookmarks
Title block
A property consists of a property name (for example, Part
Value or Part Reference) and an associated value (for
example, TIP31C or Q2). For example, part properties
define the name, value, reference designator, and other
information for each part in your design.
In Capture you can edit property values, create or delete
properties, or cause the properties to be displayed on the
schematic page.
Use one of three editors to edit properties:
The Browse spreadsheet editor, as described on
page 2-31.
The property editor, as described on page 2-34.
The Package Properties spreadsheet editor, as described
on page 45.
capug.book Page 30 Tuesday, May 23, 2000 12:08 PM
Editing properties
31
Instance and occurrence properties
Since Capture allows for complex hierarchical design
structures (as discussed in Chapter 6, Design structure),
each of the objects listed above can exist as instances or
occurrences.
In complex hierarchical designs, a schematic page can be
referenced (or reused) at several points in the design. An
instance refers to the object that is placed on the defining
schematic. An occurrence represents the use or reuse of
that instance within a design. When you edit properties
for an object, you can edit the instance, or you can edit a
particular occurrence of that instance.
Instance properties
An instance property is a user property applied to the
placed instance of a part or symbol in the design. This
includes PCB Footprint, Value, and Name properties of
each placed part or symbol in a design. The instance
property overrides the library definition.
An instance property will shine through to all
occurrences of that instance unless it is overridden by
occurrence properties. A change using any of the tools,
like Annotate, also may update the instance property.
Occurrence properties
An occurrence property is a user property applied to
multiple occurrences of place instances of parts or
symbols in a design. The occurrence property overrides
the instance property definition.
The spreadsheet editors expand to display occurrence
properties if values are different from the instance value.
To quickly hide or display all the occurrence properties,
press and hold the C key while clicking on one of the
plus (+) symbols in the property editor.
A change using any of the tools, like Annotate, also may
update the instance property.
capug.book Page 31 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
32
The Browse spreadsheet editor
You display the Browse spreadsheet editor from the
project managers Edit menu, the schematic page editor,
or the part editor. The particular Browse spreadsheet that
you display depends on the object you select from the
Browse pull-right menu. The options include:
Hierarchical ports
Off-page connectors
DRC markers
Bookmarks
Part (including hierarchical block) occurrences
Net (including constituent nets within a bus)
occurrences
Pin properties
Title block occurrences
Flat nets
The Browse spreadsheet editor browses the entire design
for the objects you select, then displays their properties.
Each property appears as a column heading in the
spreadsheet. Each row is an object located by the editor.
It is important to note that, in the Browse spreadsheet
editor you can only edit properties for occurrences. The
only exception being in the part editor, where you can
only edit instances. To edit instance properties, you must
use the property editor discussed in The property editor on
page 2-34.
Figure 13 Browse sprea
d
s
h
eet e
d
itor
capug.book Page 32 Tuesday, May 23, 2000 12:08 PM
Editing properties
33
To create a new property in the Browse spreadsheet editor
1In the first column of the Browse spreadsheet, select
the object or occurrence for which you want to create
the new property.
2From the Edit menu, choose Properties. Capture
displays the object in a new Browse spreadsheet
window.
3Click New. Capture displays the New Property dialog
box.
4Enter a name and value for the new property, then
click OK. Capture adds the property to the object or
occurrence and displays the new property in the
original Browse spreadsheet.
To copy a value from one property to another property in the
Browse spreadsheet editor
1In the first column of the Browse spreadsheet, select
the object or occurrence that has the property with the
value you want to copy.
2From the Edit menu, choose Properties. Capture
displays the object in a new Browse spreadsheet
window.
3Select the cell that contains the value you want to
copy.
4Click Copy.
5Select the cell that you want to contain the copied
value.
6Click Paste. Capture pastes the value into the selected
cell.
capug.book Page 33 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
34
To remove a user-defined property in the Browse spreadsheet
editor
1In the first column of the Browse spreadsheet, select
the object or occurrence that has the property you
want to remove.
2Select the column heading for the property you want
to remove.
3Click Remove. Capture removes that property from
the object.
To replace property values
1Select the objects whose properties you want to edit.
Note that the objects must be of the same type (for
example, all pins or all hierarchical ports); otherwise,
the Properties command is grayed out.
2From the Edit menu, choose Properties. The Browse
spreadsheet appears.
3Double-click on a cell holding the value you wish to
replace, then enter the new value.
4Click the copy button.
5Select the cells that are to receive the replacement
value.
6Click the Paste button. The replacement value appears
in the selected cells.
7Click the OK button to close the Browse spreadsheet.
Note Some properties cannot be removed
as they are essential for creating a netlist.
You can only remove user-defined
properties.
Note If you remove a property from an
occurrence for which there is a defined
instance property, the occurrence property
is not removed, but rather, the instance
property value shines through to the
occurrence. In order to remove an instance
property you must use the property editor.
For more information about instance and
occurrence properties see The property
editor on page 2-34.
capug.book Page 34 Tuesday, May 23, 2000 12:08 PM
Editing properties
35
The property editor
You display the property editor either by selecting items
on a schematic page, then choosing Properties on the Edit
or popup menu, or by simply double-clicking on an item
in the schematic page editor.
The property editor allows you to edit properties for
instances or occurrences of the following objects:
Parts (including hierarchical blocks)
Nets (including constituent nets within buses)
Pins
Title blocks
Globals
Ports
Aliases
The property editor is constrained such that it can only
edit instances or occurrences on the active schematic page.
To browse and edit properties for an entire design, see The
Browse spreadsheet editor on page 2-31.
Note Globals are power and ground
symbols, or any other objects that behave
like power and ground.
capug.book Page 35 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
36
The property editor window
The properties that appear in the property editor depend
on the items selected in the schematic page. Also, these
properties depend on the tab selection at the bottom of the
property editor. For example, if the Parts tab is active, the
properties for selected parts appear in the property editor.
Figure 14 Property editor
Each column in the property editor is a placeholder that
you can use to add properties.
Each row is an instance or occurrence. Occurrence rows
appear in yellow below their associated instance row.
They only appear if one or more occurrence property
values are different from the instance property values and
you expand the instance by clicking the plus sign (+) to the
left of the instance name.
The cells in the property editor show the property values
for each instance or occurrence. If a white cell contains a
cross-hatch pattern, the corresponding property does not
have an instance value, causing the library definition to
shine through to the instance. If a yellow cell contains a
Note When you first start the property
editor all instance properties are displayed.
Occurrence properties are displayed only if
they have their own values assigned to
them (independent of the instance property
values).
Instance name
Property names Filter drop-down list
Item selection tabs
Occurrence
Property value
schematic name:page:reference
hierarchical path:reference
capug.book Page 36 Tuesday, May 23, 2000 12:08 PM
Editing properties
37
cross-hatch pattern, the corresponding property does not
have an occurrence value, causing the instance property
value to shine through to the occurrence.
New Column or New Row Displays the Add New
Column dialog box or the Add New Row dialog box,
depending on the property editor orientation. These
dialog boxes add a new property column or row,
respectively. To add the property to an object, you must
enter a property value for the object.
Apply Applies the changes in the property editor to the
schematic page. The Apply button does not dismiss the
property editor. You can also apply the changes to the
schematic page by closing the property editor.
Display Opens the Display Properties dialog box to set
the display options of the selected property and its value.
You cannot display properties of an occurrence property
using the Display Properties dialog box.
Delete Property Deletes the property, if editable, from
the selected object or objects. If you select all of a
propertys cells and click the Delete Property button, the
property will be removed from the selected objects but
will remain in the filter. This is indicated by the
cross-hatch pattern that appears in the cell.
Filter by Specifies a filter by which you can view
objects. Use the filters available in the drop-down list to
constrain the available properties. Each filter is a set of
properties that are typically useful for particular project
types. For example, the Actel Designer Part/Net
Properties filter includes properties that are useful for
constraining a PLD project for integration with Actels
Designer software. The Capture filter displays common
schematic capture properties available to most parts. The
Layout filter displays properties needed to send a design
to Orcad Layout. The <Current properties> filter causes
N
ote
Y
ou can p
i
vot t
h
e property e
di
tor
spreadsheet. Instances and occurrences
appear in columns across the top and
properties appear in rows. This may be
advantageous if your selected object or
objects have several properties. See To
pivot the property editor
spreadsheet on page 2-38.
Note Properties that are not editable
appear in italics.
capug.book Page 37 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
38
the property editor to display all properties that currently
exist for the selected item. For more information, see The
property editor Filter menu on page 2-39.
Parts tab Displays the parts of the selected objects,
including hierarchical blocks.
The Graphic property column provides the option to
toggle the display of the part between Normal and
Convert view. When you click the Graphic cell, a down
arrow indicates a drop-down list where you can select a
different view.
Schematic Nets tab Displays the schematic nets of the
selected objects, including constituent nets within buses.
Pins tab Displays the pins of the selected objects,
including hierarchical pins in hierarchical blocks.
Title Blocks tab Displays the title blocks of the
selected objects. With this tab, you can add a property to
the Title Block instance on a schematic page that displays
the full hierarchical path to the schematic.
Globals tab Displays selected globals for simultaneous
editing of multiple names.
Ports tab Displays the source symbol, source library,
and type of port. This tab provides for simultaneous
editing of multiple ports.
Aliases tab Displays color, font, name, and rotation of
net aliases. Use this tab to edit multiple aliases at one time.
capug.book Page 38 Tuesday, May 23, 2000 12:08 PM
Editing properties
39
To pivot the property editor spreadsheet
1Right-click the empty cell in the top-leftmost position
of the spreadsheet.
2From the pop-up menu, choose Pivot.
To display or hide all occurrence properties
1To display all occurrence properties, press and hold
the C key while clicking on one of the plus (+)
symbols in the left-most column.
2To hide all occurrence properties, press and hold the
C key while clicking on one of the minus (-) symbols
in the left-most column.
To move columns in the property editor
1Select the column you want to move by clicking on its
title cell.
2Drag the column to the new location.
To sort columns in the property editor
1Right-click on the column heading. A pop-up menu
appears.
2Choose Sort Ascending or Sort Descending.
Note The Find command searches down
columns in the spreadsheet, regardless of
the spreadsheet orientation.
Note If the spreadsheet is pivoted, use
these steps to move rows.
capug.book Page 39 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
40
The property editor Filter menu
The property editor filter is a powerful tool with which
you can show or hide properties on selected objects. You
can use the pop-up Filters menu on the spreadsheet to
view the status of a property or edit columns, tabs, or the
entire property editor spreadsheet.
You can add, delete, or change any filter except the
<Current properties> filter. The <Current properties>
filter displays all properties as undefined until you create
or select another filter.
When you create a new filter, all properties appear
undefined, just as in the <Current properties> filter. If you
right-click a column heading and select Filters from the
pop-up menu, you will see that each property is
Undefined, and the filter specifies Show Undefined.
Your results will be more reliable if you use the property
editor Filters menu to make changes rather than editing
the PREFPROP.TXT file manually.
Changes to the filters are saved to PREFPROP.TXT when
you close the spreadsheet. If you need to retrieve the
original version, you can copy PREFPROP.TXT from the
Orcad installation CD in the Capture directory.
The first four choices on the Filter menu apply to the
appearance of a particular tab and column.
Show The selected column always appears when you
use the filter, unless the filter is inverted.
Hide The selected column never appears when you use
the filter, unless the filter is inverted.
Optional The selected column only appears if the
property exists on one or more objects when you use this
filter.
capug.book Page 40 Tuesday, May 23, 2000 12:08 PM
Editing properties
41
Undefined The selected property is not defined. It isnt
included or excluded from the filter.
You can control the display of undefined properties on
individual tabs with the next two choices on the Filter
menu. Select any combination of the two.
Show Undefined Specifies that any undefined
property columns that are selected appear when you use
the filter. However, if you also select Invert Filter, these
same selections will not appear.
Defined properties appear at the beginning of the
spreadsheet (toward the left side) when you select this
option.
Invert Filter Shows hidden property columns when
you use the filter. Conversely, it will hide any property
columns that you have specified to show. For example, if
a property is optional and does not exist on any objects,
you can use Invert Filter to show the property.
The last two choices on the Filter menu affect all tabs on
the property editor.
Add Filter Add a new filter to all tabs. The default of a
new filter is to show all properties as undefined
Remove Current Filter Delete the filter currently
displayed in the Filter by list box. You cannot undo this
operation.
capug.book Page 41 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
42
To create a new filter in the property editor
1Right-click any column heading in the spreadsheet.
2Point to Filters in the pop-up menu and choose Add
Filter.
3Type the new filter name in the Add Filter dialog box
and click OK. The new filter is saved in
PREFPROP.TXT when you close the property editor.
To edit a filter
1Select a filter from the Filter by drop-down list. The
appearance of the properties on the spreadsheet may
change when you change the filter.
2Right-click any column heading and point to Filters in
the pop-up menu.
3Use the Filters menu choices to change the property
definitions and appearance of the spreadsheet.
capug.book Page 42 Tuesday, May 23, 2000 12:08 PM
Editing properties
43
Using the property editor
When editing properties in the property editor, it is
important to remember a few key points:
Property values that are applied to instances will
shine through to all occurrences of those instances,
unless an occurrence has a value (independent of the
instance value) for a particular property.
Occurrence property values override instance
property values.
When you delete an instance property, that property
will no longer shine through to its occurrences.
Deleting a property value from an occurrence causes
the instance property value to shine through to that
occurrence.
Library definitions will shine through to the
instance and occurrence of the object only if the
instance or occurrence value is unedited.
To create a new property in the property editor
1In the schematic page editor, select the object(s) for
which you want to create the property.
2From the Edit menu, choose Properties. Capture
displays the property editor.
3Click the New Column or the New Row button.
Capture displays the Add New Column dialog box or
the Add New Row dialog box.
4Enter a name for the new property and click OK.
Capture adds the new property to the property editor
and to all instances and occurrences currently
displayed therein.
5Enter values for the property as described in To edit a
property value in the property editor.
capug.book Page 43 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
44
To edit a property value in the property editor
1In the property editor, select the cell that contains the
value you want to change.
2Right-click and choose Edit from the pop-up menu.
The Edit Property Values dialog box appears.
3Type in the new value and press R. Note that
changing an instance property value causes that value
to shine through to all occurrences of the instance
that do not have a value independent of the instance.
To edit the a property value for all instances and occurrences
currently displayed in the property editor
1In the property editor, click the top-leftmost cell to
select the entire spreadsheet.
2Right-click and choose Edit from the popup menu.
3Select a property cell in the Edit Property Value dialog
box spreadsheet.
4Type the new value for the property and click OK. The
new property value appears on the spreadsheet for all
selected objects.
To delete a property in the property editor
1Select the column of the property you want to delete.
2Click the Delete Property button. The property is
removed. (The property column remains in the
display. To see that the property is deleted, leave the
property editor and then return to it.)
Note Some property values (those that
have particular significance to the design
database) cannot be edited. Properties that
are not editable appear in italics.
Note Some property values (those that
have particular significance to the design
database) cannot be deleted.
capug.book Page 44 Tuesday, May 23, 2000 12:08 PM
Editing properties
45
To display a property on the schematic page
1In the property editor, select the instance property
cells you want to display, then click the Display
button. Capture displays the Display Properties
dialog box.
2Complete the dialog box as desired, then click OK.
Capture displays the property on the schematic page
for all instances currently displayed in the property
editor.
For information on the Display Properties
dialog box, see the Capture online help.
Note Although you can only set the display
for instances, the property value that
appears on the schematic page is that of the
particular occurrence.
capug.book Page 45 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
46
The Package Properties spreadsheet editor
You can edit package properties using the Package
Properties spreadsheet editor. The Package Properties
spreadsheet editor is available in the part editor while in
Package View. Use the Properties command on the Edit
menu to display this spreadsheet. The spreadsheet
displays all the package information on pins.
Figure 15 Package Properties spreadsheet editor
The Package Properties spreadsheet editor is similar to the
Browse spreadsheet editor with the following differences:
The Package Properties spreadsheet editor doesnt
have New or Remove buttons. You cannot add
properties to a package or remove existing properties.
The Package Properties spreadsheet displays all of the
pins in the package, regardless of what is selected in
the part editor.
The Package Properties spreadsheet displays the
PinGroup and Ignore properties. These do not show
up in the Browse spreadsheet editor.
The Package Properties spreadsheet has an Update
button and a Validate button.
capug.book Page 46 Tuesday, May 23, 2000 12:08 PM
Editing properties
47
Update button Use this to update the properties of all
the pins in the package. This is useful if you change a
property on one pin and need to change this property on
the same pin in the other parts of the package. For
example, say you have a four-part package and each part
in the package has a pin named IN. If you change this pin
from a passive pin to an input pin the A package part, you
could use Update to change the property for the IN pin in
the B, C, and D package parts. The Update button updates
all pins at once, without requiring that you click OK.
Validate button Use this button to check for duplicate
pins. For example, suppose you have a pin 1, and then
change another pin to pin 1. Using Validate detects the
duplicate. The Validate button checks for duplicate pin
numbers without requiring that you click OK.
capug.book Page 47 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
48
Moving and resizing graphic
objects
For some objectssuch as wires, buses, lines, ellipses,
rectangles, and so onyou can edit the objects size and
shape by clicking on it and dragging its resize handles.
Before you can move or resize a graphic object, you must
first select it. A selected object has resize handles that you
use to change the size of the graphical object.
To resize and move objects
1Select the object to resize or move.
2To resize the object, press the left mouse button on a
resize handle, and drag the handle until the object is
the size you would like it. Release the mouse button.
or
To move the object, press the left mouse button
anywhere on the objectexcept on a resize handle
and drag the object until it is where you want it.
Release the mouse button.
3To deselect the object, click in an area where there are
no parts or objects.
Note For descriptions of other ways to
manipulate objects, see Chapter 8, Adding
and editing graphics and text.
capug.book Page 48 Tuesday, May 23, 2000 12:08 PM
Undoing, redoing, and repeating an action
49
Undoing, redoing, and repeating
an action
You use the Undo command to undo your action. To
repeat an edit action, use the Repeat command. For
example, you might move a selected object five grid units,
then realize you also need to move a different object the
same distance. Select the second object, then from the Edit
menu, choose the Repeat command. You can use the
Undo, Redo, and Repeat commands with the following
actions:
Placing objects
Deleting objects (except for the Repeat command)
Copying objects
Moving objects
Resizing objects
Rotating objects
Mirroring objects
To undo an action
1From the Edit menu, choose Undo.
To reverse an undone action
1From the Edit menu, choose Redo.
To repeat a command
1Perform the command once.
2From the Edit menu, choose Repeat.
T
ip You can use the Repeat command to
align objects or to quickly create repetitive
structures such as buses.
capug.book Page 49 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
50
To repeat a copy operation
1Select an object on a schematic page.
2Press C and drag the object to a new location. This
creates a copy of the object. Leave the object selected.
3From the Edit menu, choose Repeat. The pointer
repeats the relative move in step 2 and an additional
object is placed.
capug.book Page 50 Tuesday, May 23, 2000 12:08 PM
Using the Accessories menu
51
Using the Accessories menu
You can use extensions to the Orcad-supplied
functionality of Capture if you purchase software
developed by associates of Orcad. These associates create
.DLL files that address specific Capture functionality,
such as customized netlist creation. The associates
configure their .DLL files so that they are listed as menu
choices on the Accessories menu, available in either the
project manager window or the schematic page editor
window.
capug.book Page 51 Tuesday, May 23, 2000 12:08 PM
Chapter 2 The Capture work environment
52
capug.book Page 52 Tuesday, May 23, 2000 12:08 PM
Starting a project
3
A project file (.OPJ) stores pointers to a single design file
(.DSN), and can also contain libraries, VHDL files, and
output reports associated with the design file. A design
file contains one or more schematic folders, in which there
are one or more schematic pages. A design file also
contains a design cache, which is like an embedded
libraryit contains a copy of all the parts and symbols
used on the schematic pages. When a design is saved with
the project file, information from the various Tools dialog
boxes is also saved in the project file.
Note Parts reside in a library the same
w
ay schematic pages reside in schematic
folders. Symbols and title blocks also reside
in libraries. A project can use any number
of libraries, and a library can be included in
any number of projects. However, a project
may have only one design (.DSN).
capug.book Page 51 Tuesday, May 23, 2000 12:08 PM
Chapter 3 Starting a project
52
Creating new projects, designs,
libraries, and VHDL files
Capture includes a project wizard that provides an easy
method for creating a project, complete with library and
simulation resources.
Creating a project does not create a design within the
project. A new design inherits characteristics from the
settings in the Design Template dialog box, so you should
always check those settings before you create a design.
A newly created project contains a schematic folder that
holds one schematic page. After you create a schematic
folder, you can move existing pages into it, and you can
create new pages in it.
Libraries store parts, symbols, custom title blocks, as well
as schematic folders and the schematic pages contained in
them. With Capture, you can have as many libraries as
you wish to suit any purpose, and you can specify the
name and storage location of your library. Each library is
available to each project.
To create a new project
1From the File menu, choose New, then choose Project.
The New Project dialog box appears.
2Type a name for your new project in the Name text
box.
3Use the Browse button to select a new directory.
4Select a project type in the Create a New Project Using
group box, and click OK. Capture provides the
following project types:
Analog or mixed signal circuitselect this type of
project if you intend to use your design with
PSpice. Follow the guidance of the Analog
Mixed-Mode Project wizard to add the
appropriate files to your project.
Note T
h
e project types avai
l
a
bl
e to you
w
ill depend upon which Orcad programs
y
ou have installed. As a minimum, you will
have the option to create a PC Board or
Schematic project type.
capug.book Page 52 Tuesday, May 23, 2000 12:08 PM
Creating new projects, designs, libraries, and VHDL files
53
PC boardselect this type of project if you intend
to use your design with Orcad Layout. Follow the
guidance of the PCB Project Wizard to add the
appropriate files to your project.
Programmable logicselect this type of project if
you intend to use your design with an FPGA or
CPLD EDA tool. Follow the guidance of the
Programmable Logic Project Wizard to add the
appropriate files to your project.
Schematicselect this type of project if none of the
other project types apply. Using this option,
Capture creates a basic project containing only the
design file.
To create a new design
1From the File menu, choose New, then choose Design.
2The design opens in a new PCB project manager and a
new schematic page displays.
The first time you save a new design, the Save As dialog
box appears, giving you the opportunity to specify a drive
and replace the system-generated name.
To create a new schematic page
1On the File tab of the project manager, select the
schematic folder that requires a new schematic page.
2Click the right mouse button and choose New Page
from the pop-up menu. A new schematic page
appears within the schematic folder you selected in
step 1.
To create a new library
1From the File menu, choose New, then choose Library.
2The library opens in the project manager and a Library
Cache folder is added to the project manager, or the
library opens in the existing open project manager and
a library cache is added.
Note A project cannot have more than one
design (.DSN) file. If you try to add a
second .DSN file to your project, the
Overwrite dialog box appears, asking if
y
ou want to replace the existing design.
For information on how to create parts for
inclusion in a library, see Chapter 12,
Creating and editing parts.
capug.book Page 53 Tuesday, May 23, 2000 12:08 PM
Chapter 3 Starting a project
54
To create a new VHDL file
There are two ways to create a new VHDL file in Capture:
1From the File menu, choose New, then choose VHDL
File.
2A VHDL file opens in Captures VHDL programmers
editor.
Or
1With the project manager active, choose New VHDL
File from the Design menu. The file opens in the
VHDL programmers editor and a dialog box appears,
asking if you want to add the file to the project.
2Choose the Yes button to add the file to the project that
is currently open. The Save As dialog box appears.
3Select a directory for the file and supply a filename. By
default, the VHDL files name is VHDLn.VHD (where
n is an integer indicating the number of .VHD files
created in the current session).
4Choose the Save button. Capture saves the file and
places it in the Design Resources folder of your
project.
Note If you choose the No button, Capture
does not add the VHDL file to your project
and you must save it yourself at a later
point in time.
capug.book Page 54 Tuesday, May 23, 2000 12:08 PM
Opening existing projects, designs, libraries, and VHDL files
55
Opening existing projects,
designs, libraries, and VHDL files
You can open an existing project, design, library or VHDL
file. Existing schematic pages can only be opened from
within designs and libraries.
To open an existing project
1From the File menu, point to Open, then choose
Project. The Open Project dialog box displays.
2Select a project (.OPJ) or type the name in the File
name text box, then choose the Open button. The
project opens in the project manager.
To open an existing design
1From the File menu, point to Open, then choose
Design. The Open Design dialog box displays.
2Select a design (.DSN) or type the name in the File
name text box, then choose the Open button. The
design opens in the project manager.
To open an existing schematic page
1In the project manager, select the File tab and
double-click the icon of a schematic folder; this
expands the folder and reveals the schematic pages it
contains.
2Double-click on the icon of the schematic page you
want to open. The schematic page opens in a
schematic page editor window.
T
ip The four files that were last opened are
listed at the bottom of the File menu. To
open one of these files, select it from the
File menu.
Figure 16 Open project,
d
esign, an
d
schematic page
capug.book Page 55 Tuesday, May 23, 2000 12:08 PM
Chapter 3 Starting a project
56
To open an existing library
1From the File menu, point to Open, then choose
Library. The Open Library dialog box displays.
2Select a library (.OLB) or type the name in the File
name text box, then choose the Open button. The
library opens in the project manager.
To open an existing VHDL file
1From the File menu, point to Open, then choose VHDL
File. The Open VHDL File dialog box displays.
2Select a VHDL file (.VHD) or type a name in the File
name text box, then choose the Open button. The
VHDL file opens in Captures text editor.
Figure 17 Open library
Figure 18 Open VHDL file
capug.book Page 56 Tuesday, May 23, 2000 12:08 PM
Working with files in a project
57
Working with files in a project
Using the project manager, you can add or delete project
files. You can add any file to your project, including
libraries and VHDL files. Files not in ASCII format, or a
Capture generated format, may not appear as expected
when opened in Capture.
To add a file to your project
1In the project manager, select the folder to which you
want to add a file.
2From the Edit menu, choose Project. The Add File to
Project Folder dialog box displays.
3Select the file you want to add and choose the Open
button. The file is added to the project.
Or
1Drag the file from the Windows Explorer into the
folder in the project manager.
To delete a file from a project
1In the project manager, select the file you want to
delete.
2Press the D key. The file is removed from the
project.
Note You can also add files to your project
interactively. When you create a design
using the New command on the File menu,
it is placed in the project managers Design
Resources folder.
Caution You will not be given a chance to
cancel this process after you press the
D key. If you delete a file by mistake,
y
ou will have to add it back to the project.
capug.book Page 57 Tuesday, May 23, 2000 12:08 PM
Chapter 3 Starting a project
58
Saving projects, designs, and
libraries
When the project manager window is active, you can save
a new or existing project, design, or library. The Save
command saves all open documents referenced by the
project, as well as the project itself.
A Capture design file (.DSN) is associated with a project
file (.OPJ). Each time you use the Save As command from
the File menu to save a design file to another name or
directory, you should also use Save As for the project file.
The Save As command saves files depending on what you
have selected in the project manager.
If one or more designs or libraries are selected,
Capture prompts you to save each file in turn.
If no top-level folders (Design Resources or Outputs)
are selected, and items other than designs or libraries
are selected, the Save As command is unavailable.
If no designs or libraries are selected in the project
manager, Capture prompts you to save the project.
To save a new design or library
1With the design or library selected in the project
manager, from the File menu, choose Save. The Save
As dialog box displays.
2Enter a name for the design or library in the File name
text box, specify a location, then choose the Save
button.
The design or library is saved, and the project manager
remains open. When you close the project, Capture
prompts you to save the project file.
Note To avoid overwriting a design file
w
ith a misnamed project file, type in the
filename without a file extension. Capture
automatically saves the file with the correct
file extension.
T
ip To protect your work in the event of a
system crash or power outage you can
enable Auto Recovery, and set the interval
at which your design, library, or VHDL file
is saved. For information about the Auto
Recovery option, see Setting miscellaneous
options on page 4-73.
Note If you choose Save when a schematic
page window is active, only that pages
design is saved, not the entire project.
However, when you attempt to close the
project, a dialog box asks if you want to
save any project files that have been edited
but not yet saved.
capug.book Page 58 Tuesday, May 23, 2000 12:08 PM
Closing a project
59
To save an existing project
1With the Design Resources or Output folder selected,
choose Save from the File menu.
The project is saved, and remains open in the Capture
session frame.
Using the Save As command
The following process saves a .DSN file and a .OPJ file into
the same directory so you can continue editing the current
project without altering the original files.
1In the project manager, select the design file.
2From the File menu, choose Save As.
3Change the drive and directory as appropriate, then
select the file name and click Save.
4Select the Design Resources folder.
5From the File menu, choose Save As.
6Change the drive and directory as appropriate, then
select the file name and click Save.
Closing a project
When the project manager window is active, you can close
a project without quitting Capture, or you can close and
save your project as you quit.
To close a project
1From the project managers File menu, choose Close
Project.
When you close a project, a dialog box displays, asking if
you want to save your changes.
To quit Capture
1From the project managers File menu, choose Exit.
capug.book Page 59 Tuesday, May 23, 2000 12:08 PM
Chapter 3 Starting a project
60
When you choose the Exit command, a dialog box
displays, asking if you want to save your changes.
Choose Yes to save the specific document within
the project.
Choose Yes All to save all documents in the
project.
Choose No to close the document without saving
it.
Choose No All to close all open documents
without saving them.
Choose Cancel to abort closing the project.
capug.book Page 60 Tuesday, May 23, 2000 12:08 PM
Archiving a project
61
Archiving a project
When the project manager window is active, you can
archive a project. Archiving saves all files related to your
project in the specified directory. Specifically, this
command saves your project files (*.OPJ), design files
(*.DSN), and library files (*.OLB) in the Design Resources
folder. You can include output files and library files, like
*.OLB files in the Library folder and *.VHD files.
To archive a project
1Make sure that the project you want to archive is
active.
2From the project managers File menu, choose Archive
Project. The Archive Project dialog box appears.
3Select the types of additional files you want archived
with your project. If you dont select any of the options
(Library files, Output files, Referenced projects),
Capture automatically archives your project (*.OPJ)
and design files (*.DSN).
4Enter or browse to the directory in which you want to
archive your project.
5Click OK. Capture archives your project with all the
selected external files to the specified directory. The
working directory does not change to the archive
directory.
Note Archive Project archives the
simulation profiles and the local files
(*.LIB, *.STL, and *.INC files) along with
PSpice projects. The Output files option
does not archive simulation output like
*.DAT and *.OUT files.
capug.book Page 61 Tuesday, May 23, 2000 12:08 PM
Chapter 3 Starting a project
62
capug.book Page 62 Tuesday, May 23, 2000 12:08 PM
Setting up your project
4
Capture provides different levels of configuration. Using
commands on the Options menu, you can:
Customize the working environment specific to your
system (using Preferences).
Create default settings for new designs (using Design
Template). These settings stay with the design as
design properties even if it is moved to another system
with different preferences.
Override settings in individual designs (using Design
Properties) or individual schematic pages (using
Schematic Page Properties).
Regardless of which Capture window is active, the
Options menu has a Preferences command and a Design
Template command. In addition, the Options menu
contains commands specific to the current active window.
For example, the project managers Options menu
contains the Design Properties command, while the
schematic page editors Options menu contains the
Schematic Page Properties command.
capug.book Page 63 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
64
The settings in the Preferences dialog box determine how
Capture works on your system, and persist from one
Capture session to the next because they are stored in the
Capture initialization (.INI) file on your system. If you
pass projects to others, they wont inherit your
Preferences settings. This means you can set colors, grid
display options, pan and zoom options, and so on to your
liking and be assured that your settings will remain, even
if you work on a project created on another system.
The Design Template dialog box determines the default
characteristics of all the projects created on your system.
Because a new project inherits characteristics from the
current Design Template settings, its a good idea to check
the settings before you create a new project.
Once you begin working on a project, you can customize
its particular characteristics by choosing Design
Properties from the Options menu when you are in the
project manager, or Schematic Page Properties when you
are in the schematic page editor.
capug.book Page 64 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
65
Defining your preferences
The options that you define in the tabs of the Preferences
dialog box affect how Capture works with your projects.
Choose Preferences from the Options menu to access the
Preferences dialog box.
Colors/Print. Set up colors for objects such as off-page
connectors, hierarchical blocks and ports, text, title
blocks, and so on, and specify which objects will be
printed or plotted. You can also change the
background color and the color of the grid.
Grid Display. Select dots or lines for your grid, and
whether to display or print your grid. You can select
whether to have your pointer snap to grid as you place
objects. You can set these options independently for
the schematic page editor and the part editor.
Pan and Zoom. Define how you want autoscrolling to
work, and what the zoom factor should be. You can set
these options independently for the schematic page
editor and the part editor.
Select. Define whether you want to select objects
enclosed by a selection rectangle or objects inside and
intersecting a selection rectangle, the maximum
number of objects to display at high resolution while
dragging, and whether to show the tool palette. You
can set these options independently for the schematic
page editor and the part editor.
Miscellaneous. Define the default fill, line style and
width, and color for graphic objects, define the font
used in the project manager and session log, render
TrueType fonts with strokes (for printing and
plotting), and set whether to auto recover your project
and how often. In addition, you can enable intertool
communication, which is the method that Capture
uses to communicate with other Orcad software, such
as Orcad Layout.
Text Editor. Define which (if any) VHDL keywords
are highlighted, and the font and tab settings used
within the text editor.
capug.book Page 65 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
66
Defining colors/print options
You control the color in which different schematic page
objects display by using the Colors/Print tab in the
Preferences dialog box.
Figure 19 Colors/Print tab of the Preferences dialog box
To define if an object is printed or plotted
1From the Options menu, choose Preferences, then
choose the Colors/Print tab.
2Select the check box by the color for the object to be
printed or plotted. Clear the check box for the object to
not be printed or plotted. Objects are always displayed
on your screen, regardless of the setting of their check
boxes.
capug.book Page 66 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
67
To define an objects color
1From the Options menu, choose Preferences, then
choose the Colors/Print tab.
2Click the left mouse button on the color of an item. The
color palette window opens.
3Select a new color. Click OK to dismiss the color
palette.
4Click OK.
Graphics objects (lines, polylines, and arcs) use the colors
specified by Miscellaneous tab. If the color options in the
Miscellaneous tab are set to Default color, then Capture
uses the color specified for graphics by the Colors/Print
tab.
Note The color that you select for Title
Block is also the color used for borders and
g
rid references.
capug.book Page 67 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
68
Controlling the grid
You can control whether Capture displays a grid
independently in the schematic page editor and the part
editor, and whether the grid uses dots or lines. You can
also specify whether the pointer snaps to grid in each
editor.
Figure 20 Grid Display tab of the Preferences dialog box
To control the grid
1From the Options menu, choose Preferences, then
choose the Grid Display tab.
2For the schematic page editor and the part editor,
specify:
Whether to display the grid.
Whether the grid uses dots or lines.
Whether the pointer snaps to grid as you place
objects.
3Click OK.
Caution If you disable the Pointer
snap-to-grid option while you are drawing,
be sure to enable it before you place
electrical objects. Otherwise, your part pins
may be placed off-grid, making it difficult
to connect them properly.
T
ip You can also show or hide the grid
using the Grid command on the View menu
in the schematic page editor or the part
editor.
T
ip You can toggle the snap-to-grid using
the snap-to-grid toolbar button.
capug.book Page 68 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
69
Setting pan and zoom
When you have an object attached to the pointer and you
move the pointer near the edge of the window while
holding the left mouse button down, the display changes
to a different region of the document. This change is called
panning. The display automatically pans only if you hold
the left mouse button down whether or not an object is
attached to the pointer; otherwise, you must use the
windows scroll buttons to view a different region of the
document. You configure the percent by which the
display changes using the Auto Scroll Percent setting.
When you zoom in or out, the view changes by the zoom
factor. You can define pan and zoom settings for the
schematic page editor and the part editor independently.
Figure 21 Pan and Zoom tab of the Preferences dialog box
capug.book Page 69 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
70
To configure zoom factor and auto scroll percent
1From the Options menu, choose Preferences, then
choose the Pan and Zoom tab.
2For the schematic page editor and the part editor, set
these options:
Zoom Factor. Enter an integer to indicate the
magnification or reduction of the objects shown in
the window when you zoom in or zoom out. This
number is a multiplier for each time you zoom in
or out.
Auto Scroll Percent. Enter the percent of the
windows horizontal or vertical dimension by
which the display will scroll when the pointer
approaches the edge of the window with an object
attached.
3Click OK.
T
ip You can also auto scroll without an
object attached to the pointer by pressing
the left mouse button as the pointer
approaches the edge of the window.
capug.book Page 70 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
71
Defining selection options
You can specify whether objects are selected when the
selection border intersects them or if the objects are
selected only when they are completely enclosed in the
selection area. You can also change the maximum number
of objects displayed at high resolution while dragging,
and set tool palette visibility in both the schematic page
editor, and the part and symbol editor.
Figure 22 Select tab of the Preferences dialog box
To define selection options
1From the Options menu, choose Preferences, then
choose the Select tab.
2For the schematic page editor and the part editor, set
these options:
Area Select. Specify whether to select objects that
are inside and intersecting the selection border or
only objects that are fully enclosed by the selection
border.
capug.book Page 71 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
72
Maximum number of objects to display at high
resolution while dragging. If you drag more
objects than you specify here, you will see
rectangular placeholders for the objects as you
drag them.
3Click OK.
Note Capture may per
f
orm s
l
ower i
f
you
set the Maximum number of objects to
display at high resolution while dragging to
a large number.
capug.book Page 72 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
73
Setting miscellaneous options
You can specify the default fill, line style and width, and
color for graphics objects, define the font used in the
project manager and session log, render TrueType fonts
with strokes (for printing and plotting), and set whether to
enable auto recovery for your project and how often. In
addition, you can enable intertool communication, which
is the method that Capture uses to communicate with
other Orcad software, such as PSpice.
Figure 23 Miscellaneous tab of the Preferences dialog box
To set miscellaneous options
1From the Options menu, choose Preferences, then
choose the Miscellaneous tab.
2For the schematic page editor and the part editor, set
these options:
Fill Style. Select the fill pattern to be used when
drawing rectangles, ellipses, and closed shapes
drawn with the polyline tool.
You can change the fill style, line style and
w
idth, and color on graphic objects on an
individual basis once they are drawn on a
schematic page. Select the object, then
from the Edit menu, choose Properties. For
specific instructions, see Chapter 8,
Adding and editing graphics and
text.
For information about intertool
communication between Capture and
Layout, see Chapter 19, Using
Capture with Orcad Layout.
For information about intertool
communication between Capture and
PSpice, see Chapter 20, Using
Capture with PSpice.
capug.book Page 73 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
74
Line Style and Width. Select the line style and
width used for lines, polylines, rectangles, ellipses,
and arcs.
3For the schematic page editor, set this option:
Color. Select the color used for graphic objects
(rectangles, ellipses, and closed polylines).
4Set the following options:
Session Log. Select a font for display text in the
project manager and session log. If you select this
option, a standard Windows dialog box for font
selection appears. Select a font, style, and size from
the dialog box, then click OK.
Text Rendering. The text rendering options affect
how text on a schematic page appears on your
screen, and how it is printed or plotted. The
Render TrueType fonts with strokes option
displays text as a series of lines, connected to
resemble the outlines of the corresponding
TrueType letters or numbers they represent.
Enabling the Fill text option causes the text
outlines to be filled in.
Note The Default color is the color defined
in the Graphics box in the Colors/Print tab
in the Preferences dialog box.
Graphics objects use the colors specified by
Miscellaneous tab. If the color options in the
Miscellaneous tab are set to Default color,
then Capture uses the color specified by the
Colors/Print tab.
T
ip The Render TrueType fonts with
strokes option produces text that is printed
or plotted quickly, but is not as aesthetically
pleasing as TrueType text. For this reason,
y
ou may want to enable the option when
y
ou print or plot drafts of your schematic
pages, then disable the option when you
print or plot the final versions of your
schematic pages.
capug.book Page 74 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
75
Auto Recovery. Select whether to enable auto
recovery for your project and, if so, the interval
between saves. You can specify any interval
between five minutes and 120 minutes. When the
time interval is up, any design, library, or VHDL
file in your project that hasnt been saved, or has
been modified since the last save, is saved as a
temporary file (with an .ASP extension) in the
WINDOWS\TEMP\AUTOSAVE directory.
When you close your project normally, the
\AUTOSAVE directory and temporary files are
deleted. In cases of power outages or system
crashes, however, the temporary files are saved.
When you restart Capture, it loads the auto
recovered files, showing Restored in their title
bars. You must use the Save As command and
provide a filename to have an auto recovered file
overwrite the original file.
Auto Reference. Select whether to enable
automatic annotating of reference designators
when parts are placed.
Intertool Communication. Select whether to
enable intertool communication (also known as
ITC), so that you can test and display design
information using other Orcad software (such as
Orcad Layout and PSpice) in conjunction with
Capture. Capture processes its tools faster when
intertool communication is not selected.
5Click OK.
capug.book Page 75 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
76
Setting text editor options
Captures text editor options include automatic
highlighting of VHDL keywords, comments, or quoted
strings. You can also set the font, the tab spacing, and
enable or disable the highlighting feature.
Figure 24 Text Editor tab of the Preferences dialog box
To set text editor options
1From the Options menu, choose Preferences, then
choose the Text Editor tab.
2Set these options:
Syntax Highlighting. Select the color to use to
highlight VHDL keywords, comments, and
quoted strings. You can choose a different color for
each.
Current Font Setting. Click Set to change the font
setting for the text editor to values other than those
displayed.
Tab Setting Set the number of spaces to use for tabs
in the text editor.
Note The Highlight Keywords, Comments,
and Quoted Strings option must be enabled
for Capture to use the syntax highlighting
options.
capug.book Page 76 Tuesday, May 23, 2000 12:08 PM
Defining your preferences
77
3Check the Highlight Keywords, Comments, and
Quoted Strings option to have those VHDL items
highlighted in the text editor. The colors used to
highlight these items are the ones set in the Syntax
Highlighting group box.
4If you want to reset the text editor options to the
Capture default values, click the Reset button.
5Click OK.
capug.book Page 77 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
78
Setting up your project template
The options that you define in the Design Template dialog
box are the default settings for all new projects, and for
schematic pages you add to an existing project. You can
override some of these options for individual projects or
schematic pages. Some of the things you can define in the
Design Template dialog box are:
Fonts. You can define the fonts for schematic page
objects that contain text, such as part references and
values.
Title Block. You can specify the text to appear in title
block fields, as well as the path and filename of the
library containing the title block. This affects new
projects, as well as new schematic pages in existing
projects.
Page Size. You can specify whether inches or
millimeters are used as the unit of measure, the width
and height of a schematic page, and the spacing
between pins.
Grid Reference. For horizontal and vertical border
grid references, you can set the number of border grid
references to display in either direction, whether the
grid references are alphabetic or numeric, whether
they increment or decrement across the schematic
page, and how wide grid reference cells are. You can
also make the border, grid references, and title block
visible or invisible. This affects new projects, as well as
new schematic pages in existing projects.
Hierarchy. For hierarchical blocks and part instances
that have their Primitive property set to Default, you
can specify if you want Capture to treat each as
primitive (cannot descend into attached schematic
folders) or nonprimitive (can descend into attached
schematic folders).
SDT Compatibility. You can specify which Capture
properties map to which Orcad Schematic Design
Tools (SDT) part fields when saving a project in SDT
format.
capug.book Page 78 Tuesday, May 23, 2000 12:08 PM
Setting up your project template
79
Setting up fonts for new projects
You can define the fonts assigned to the text associated
with different schematic page objects in new designs. The
fonts specified here do not affect existing designs.
Figure 25 Fonts tab of the Design Template dialog box
To assign fonts used for new designs
1From the Options menu, choose Design Template,
then choose the Fonts tab.
2Click the left mouse button on the font of an item. A
standard Windows font dialog box appears.
3Select a font, font style, and size. Click OK to dismiss
the font dialog box.
4Click OK.
T
o change the fonts for an existing project,
use the Fonts tab in the Design Properties
dialog box. You can access this dialog box
by choosing Design Properties from the
project managers Options menu.
T
he default fonts were selected for optimal
compatibility with SDT. Changing these
fonts may result in less optimal text sizes
for translated projects.
capug.book Page 79 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
80
Defining title block information
There are two types of title blocks: default and optional.
You specify the information that goes into the default
title block in the Title Block tab of the Design Template
dialog box. Capture places a default title block in the
lower right corner of each schematic page (if a library
and title block name are specified), and places the
information you enter in the text fields in the Title
Block tab into the title block. This information is also
used in reports created by the commands on the Tools
menu. This affects new projects, as well as new
schematic pages in existing projects. You can set the
default title block to be visible or invisible on an
existing schematic page by changing the setting in the
Grid References tab in the Schematic Page Properties
dialog box.
You can place any number of optional title blocks
anywhere on the schematic page using the Title Block
command on the Place menu. Optional title blocks
display information that you define as property
values for the title block symbol.
Figure 26 Title Block tab of the Design Template dialog box
capug.book Page 80 Tuesday, May 23, 2000 12:08 PM
Setting up your project template
81
Capture provides default title block symbols in the
CAPSYM.OLB library. One such title block is shown
below. The text shown in curly braces acts as property text
placeholders. You can specify the value by
double-clicking on the text and supplying a value. You
can control the visibility by selecting or deselecting the
Visible check box in the Display Properties dialog box.
Figure 27 Title block
To choose a title block and define the text it contains
1From the Options menu, choose Design Template,
then choose the Title Block tab.
2In the Text group box, enter the information you want
to appear in the title block.
3In the Symbol group box, enter the path and filename
of the library containing the title block.
aThe Library Name text box can be left blank if you
are using title block from the CAPSYM.OLB
library and CAPSYM.OLB has not been moved to
a different directory from where it was installed.
bIf you are using a custom title block, then put the
full path and file name for the library in the
Library Name text box.
4Enter the exact name of the title block into the Title
Block Name text box. Symbol names are case sensitive
and space sensitive.
5Click OK.
You can access the Display Properties
dialog box by following these steps:
1Double-click on the property.
or
1Double-click the object containing the
property.
2Select the property in the property
editor, and click Display.
You can create custom title blocks and store
them in a library using the New Symbol
command from the project managers
Design menu. If you specify the name of
the custom library and title block in the
Symbol group box of the Design Templates
T
itle Block tab, the custom title block
appears in the lower right corner of each
new schematic page. See Captures online
help for specific instructions.
For Capture to automatically place the
information you entered in the text fields
into your custom title block, you must give
your custom title block the appropriate
properties. See the topic Creating a custom
title block in Captures online help for more
information.
capug.book Page 81 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
82
Setting the schematic page size for new projects
For new projects, you can specify the default unit of
measure, the default width and height of schematic pages,
and the spacing between pins. The value you enter in the
Pin-to-Pin Spacing text box defines how close together
pins are placed in the part editor. It also defines the grid
spacing (the space between grid dots or grid lines)
Figure 28 Page Size tab of the Design Template dialog box
To set up the schematic page size
1From the Options menu, choose Design Template,
then choose the Page Size tab.
2In the Units area, select the default unit of measure for
new projects. This setting only affects the schematic
page editor, not the part editor.
You can select a different unit of measure
or page size (A, B, C, D, E, and Custom if the
unit of measure is Inches; or A4, A3, A2,
A1, A0, and Custom if the unit of measure
is Millimeters) for individual schematic
pages in existing projects. Choose
Schematic Page Properties from the
schematic page editors Options menu, and
use the Page Size tab.
Caution Changing from Inches to
Millimeters resets the page sizes to their
defaults; therefore, if you make any
changes to the standard page size
dimensions, then change the units, the
page size changes are not translated
between the two types of units.
capug.book Page 82 Tuesday, May 23, 2000 12:08 PM
Setting up your project template
83
3Select the default schematic page size for new projects.
For each schematic page size (A, B, C, D, E, and
Custom if the unit of measure is Inches; or A4, A3, A2,
A1, A0, and Custom if the unit of measure is
Millimeters) you can specify the width and height. The
values that you enter in the Width and Height text
boxes become the dimensions for each page size. You
cannot change these dimensions for individual
schematic pages, although you can select a different
page size, or choose to define a custom size.
4In the Pin-to-Pin Spacing text box, specify the default
spacing between pins. The value you enter in this text
box defines how close together pins are when you
place a part on a schematic page. It also defines the
grid spacing (the space between grid dots or grid
lines). You cannot change this value for existing
projects or individual schematic pages.
5Click OK.
Note Part size will vary when copying and
pasting parts between pages with different
pin-to-pin spacings.
capug.book Page 83 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
84
Defining the grid reference
You set the borders grid references to display either
horizontally or vertically, alphabetically or numerically,
incrementally or decrementally across the schematic page,
and the width of their cells. You can also make the border,
grid references, and title block visible or invisible on the
screen and on schematic pages you print. The settings
affect new projects and new schematic pages in existing
projects.
Figure 29 Grid Reference tab of the Design Template dialog box
To define the grid reference
1From the Options menu, choose Design Template,
then choose the Grid Reference tab.
2Specify the number of border grid references, whether
they are alphabetic or numeric, whether the grid
references increment (Ascending) or decrement
(Descending) across the schematic page, and how
wide the grid reference cells are.
You can change these settings for existing
schematic pages. Choose Schematic Page
Properties from the schematic page editors
Options menu, then choose the Grid
Reference tab in the Schematic Page
Properties dialog box.
Note The size of the Grid Reference font is
tied to the width.
capug.book Page 84 Tuesday, May 23, 2000 12:08 PM
Setting up your project template
85
3For the border, title block, and grid reference, select
Displayed to have the item display on the screen or
Printed to have the item appear on schematic pages
you print. Select ANSI grid references to display the
grid references in accordance with ANSI standards
(see the glossary entry ANSI).
4Click OK.
capug.book Page 85 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
86
Defining the default hierarchy option for new
projects
For hierarchical blocks and part instances that have their
Primitive property set to Default, you can specify if you
want Capture to treat each as primitive (cannot descend
into attached schematic folders) or nonprimitive (can
descend into attached schematic folders). The Primitive
and Nonprimitive options in the Hierarchy tab of the
Design Template dialog box only affect new projects.
Note that this setting affects how the options on the Tools
menu process projects.
Figure 30 Hierarchy tab of the Design Template dialog box
To define the default hierarchy option
1From the Options menu, choose Design Template,
then choose the Hierarchy tab.
2For hierarchical blocks and parts, select Primitive or
Nonprimitive. All hierarchical blocks and part
instances that have their Primitive property set to
Default will use the setting selected here.
3Click OK.
Note You can change the hierarchy option
for existing projects using the Hierarchy tab
in the Design Properties dialog box. Choose
Design Properties from the project
managers Options menu.
For more information, see Primitive
and nonprimitive parts on
page 11-208.
capug.book Page 86 Tuesday, May 23, 2000 12:08 PM
Setting up your project template
87
Setting up compatibility with Orcads Schematic
Design Tools (SDT)
You can specify which properties Capture stores in the
eight SDT part fields when saving a project in SDT format.
In the dialog box shown below, the part fields listed on the
left are SDTs part fields. The text boxes on the right are
used to specify which of Captures properties map to the
part fields in SDT. The options in the SDT Compatibility
tab of the Design Template dialog box only affect new
projects.
Figure 31 SDT Compatibility tab of the Design Template dialog
box
To set up compatibility with Orcads Schematic Design Tools
1From the Options menu, choose Design Template,
then choose the SDT Compatibility tab.
2For each Capture property you want mapped to an
SDT part field, specify the part field to contain the
property value.
3Click OK.
Orcads Schematic Design Tools
(SDT 386+) was Orcads DOS-based
schematic capture program.
Note You can also use the part fields for
mapping netlists that use part field
information. For information on creating
these types of netlists and the combined
property strings they require, see the
Capture online help.
T
ip To change the part field to property
mapping for existing projects, use the SDT
Compatibility tab in the Design Properties
dialog box (from the project managers
Options menu, choose Design Properties).
capug.book Page 87 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
88
Changing properties of existing
projects
When you create a new project, it uses the options defined
in the Design Template dialog box. You can set the options
on existing projects using the Design Properties dialog
box (from the project managers Options menu). The
options are:
Fonts. You can define the fonts for schematic page
objects that contain text, such as part references and
part values.
Hierarchy. You can specify hierarchical blocks and
part instances whose Primitive property is set to
Default be treated as primitive (cannot descend into
attached schematic folders) or nonprimitive (can
descend into attached schematic folders).
SDT Compatibility. You can specify which Capture
properties map to which SDT part fields when saving
the design in SDT format.
Miscellaneous. You can view the project name, root
schematic folder name, creation time, and
modification time. Also, if you need to see the power
pins on a schematic page for documentation or
debugging purposes, you can display them on the
screen.
You can override other Design Template
options (page size and grid reference)
using the Schematic Page Properties dialog
box. For further information, see
Changing properties of existing
schematic pages on page 4-92.
T
o get to the Design Properties option, you
must select either the design name, a
schematic folder, or a schematic page in the
project manager.
capug.book Page 88 Tuesday, May 23, 2000 12:08 PM
Changing properties of existing projects
89
Assigning fonts
Fonts are assigned to new projects using the Fonts tab in
the Design Template dialog box. You can change fonts for
existing projects using the Fonts tab in the Design
Properties dialog box (choose Design Properties from the
project managers Options menu). When you change the
settings for the fonts in Design Properties, all affected text
which is set to the default font will be changed. If you have
assigned a unique font to any piece of text in the design,
these will not be affected by changing the default font. See
Setting up fonts for new projects on page 4-79 for more
information.
Defining hierarchy
The behavior for hierarchical blocks and part instances
whose Primitive property is set to Default (whether to act
as primitive or nonprimitive) is defined for new projects
using the Hierarchy tab in the Design Template dialog
box. You can change this behavior for individual projects
using the Hierarchy tab in the Design Properties dialog
box (choose Design Properties from the project managers
Options menu). See Defining the default hierarchy option for
new projects on page 4-86 for more information.
Using Capture with SDT
The mapping of Schematic Design Tools to Capture
properties for new projects is defined using the SDT
Compatibility tab in the Design Template dialog box. You
can change this mapping for individual projects using the
SDT Compatibility tab in the Design Properties dialog box
(choose Design Properties from the project managers
Options menu). See Setting up compatibility with Orcads
Schematic Design Tools (SDT) on page 4-87 for more
information.
capug.book Page 89 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
90
Viewing design information
Capture displays information in the Design Properties
dialog box about the .DSN file thats selected in the project
manager. On the Options menu, choose Design Properties
and select the Miscellaneous tab to open the Design
Properties dialog box and view:
The path and file name of the design.
The name of the root schematic in the design.
The format for the date in the title block. (You can click
the down arrow and select a new format.)
The creation time of your schematic page.
The last time your schematic page was modified
Figure 32 Miscellaneous tab of the Design Properties dialog box
You can also set Capture to display power pins for the
purpose of documentation. For more information, see
Viewing and connecting to invisible power pins on page 4-91.
capug.book Page 90 Tuesday, May 23, 2000 12:08 PM
Changing properties of existing projects
91
Viewing and connecting to invisible power pins
Normally, power pins are invisible and thus global.
Selecting the Display Invisible Power Pins (for
documentation purposes only) option in the
Miscellaneous tab will display the pins on the screen, and
they are still considered global. However, you can only
view the power pinsyou cannot connect to them.
To view invisible power pins without isolating them
1From the project managers Options menu, choose
Design Properties, then choose the Miscellaneous tab.
2Select the Display Invisible Power Pins option.
3Click OK.
Note To connect wires and other electrical
objects to power pins, you must make them
visible on the part or instance. Select the
part and then, from the Edit menu, choose
Properties. Select the Power Pins Visible
option and click OK. If you connect a wire or
other electrical object to a power pin made
visible by this method, that pin is isolated
from the global net.
capug.book Page 91 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
92
Changing properties of existing
schematic pages
When you add a new schematic page, the options defined
in the Design Template dialog box are used. You can
override these options on existing schematic pages by
using the options in the Schematic Page Properties dialog
box. You access this dialog box by choosing Schematic
Page Properties from the schematic page editors Options
menu. The options in the Schematic Page Properties
dialog box are:
Page Size. You can specify the unit of measure and the
page size.
Grid Reference. You can set the number of horizontal
or vertical border grid references to display, whether
the grid references are alphabetic or numeric, whether
they increment or decrement across the schematic
page, and how wide the grid reference cells are. You
can also make the border, grid references, and title
block visible or invisible.
Miscellaneous. You can view information about the
schematic page, such as creation time, modification
time, and page number.
Changing page size
For existing schematic pages, you can change the unit of
measure from Inches to Millimeters or select a different
page size. Since the width and height for each page size
(except Custom) and the pin-to-pin spacing are set in the
Design Template Page Size tab, you cannot change these
particular items in the Schematic Page Properties Page
Size tab. You can access the Schematic Page Properties
dialog box by choosing Schematic Page Properties from
the schematic page editors Options menu. See Setting the
schematic page size for new projects on page 82 for more
information.
You can override other Design Template
options (fonts, hierarchy, and SDT
compatibility) using the Design Properties
dialog box. For further information, see
Changing properties of existing
projects on page 4-88.
capug.book Page 92 Tuesday, May 23, 2000 12:08 PM
Changing properties of existing schematic pages
93
Setting up new grid references
Horizontal and vertical border grid references for new
schematic pages are set up in the Grid Reference tab of the
Design Template dialog box. You can change these
settings for existing schematic pages using the Grid
Reference tab in the Schematic Page Properties dialog box
(choose Schematic Page Properties from the schematic
page editors Options menu). See Defining the grid reference
on page 84 for more information.
Viewing miscellaneous schematic page properties
The Miscellaneous tab in the Schematic Page Properties
dialog box displays the creation time and the last
modification time of the schematic page, as well as the
page number.
Figure 33 Miscellaneous tab of the Schematic Page Properties
dialog box
capug.book Page 93 Tuesday, May 23, 2000 12:08 PM
Chapter 4 Setting up your project
94
To view miscellaneous schematic page properties
1From the schematic page editors Options menu,
choose Schematic Page Properties, then choose the
Miscellaneous tab.
2When you are done viewing the information, click OK.
capug.book Page 94 Tuesday, May 23, 2000 12:08 PM
Printing and plotting
5
To send output to a printer, a plotter, or an encapsulated
PostScript® file, use the standard Windows Print Setup,
Print Preview, and Print dialog boxes.
Printing commands can be chosen from the File menu in
the project manager, the schematic page editor, or the part
editor. You can print schematic pages, parts, or packages.
To configure a printer or plotter
1From the File menu, choose the Print Setup command.
Select an appropriate printer or plotter, or change the
printer settings if necessary, and then click OK.
Note Capture can sen
d
output to any print
driver that Windows supports. For
additional information on print drivers, see
the documentation included with Microsoft
Windows.
Note To install and remove printers and
plotters, and to set additional printing
options, see the documentation included
w
ith Microsoft Windows regarding the
Windows Control Panel.
capug.book Page 95 Tuesday, May 23, 2000 12:08 PM
Chapter 5 Printing and plotting
96
Printing or plotting schematic
pages
You can print or plot a schematic page, or several
schematic pages, from the project manager.
To print or plot a schematic page or pages
1Activate the schematic page editor window for the
page you want to print.
or
In the project manager, select the schematic page or
pages.
or
If you want to print all the pages in the design, select
the design name in the project manager.
2From the File menu, choose Print. The Print dialog box
appears.
3Select the scale, print offsets, print quality, number of
copies, and whether to print to file.
4Click OK to send the image to the output device.
capug.book Page 96 Tuesday, May 23, 2000 12:08 PM
Printing or plotting parts or packages
97
Printing or plotting parts or
packages
With the part editor active and open to a specific part or
package, you can create a print or a plot of that part or
package. You can also print a library part from the project
manager.
To print or plot a part or package
1Select the part or package you want to print in the
schematic page editor.
or
Select the library part in the project manager.
2Click the right mouse button in the project manager,
and choose Edit Part from the pop-up menu. The part
appears in the part editor.
3From the part editors View menu, choose Part to print
a part or choose Package to print a package.
4From the File menu, choose Print. The Print dialog box
appears.
5Select the scale, the print quality, and the number of
copies.
6Click OK to send the image to the output device.
capug.book Page 97 Tuesday, May 23, 2000 12:08 PM
Chapter 5 Printing and plotting
98
Printing the session log and text
editor windows
With the text editor window or session log active, you can
print the contents of the window.
To print a text editor window
1Make the text editor the active window.
2From the File menu, choose Print. The Print Range
Selection dialog box appears.
3Select whether to print highlighted text or the entire
file.
4Click OK to send the text to the output device.
To print the session log
1Make the session log the active window.
2From the File menu, choose Print. The Print dialog box
appears.
3Click OK to send the text to the output device.
capug.book Page 98 Tuesday, May 23, 2000 12:08 PM
Previewing printer or plotter output
99
Previewing printer or plotter
output
Using the Print Preview command, you can preview your
schematic page, part, or package output to check its
appearance before you commit it to paper.
To preview a schematic page
1From the File menu, choose Print Preview. The Print
Preview dialog box appears.
2Specify appropriate values in the dialog box, and then
click OK. The Print Preview display window opens
with a display of your schematic page, part, or
package.
3Use the Previous page and Next page buttons to view
other pages you intend to print.
4To zoom in, move the magnifier pointer to a specific
area and click the left mouse button.
5Choose the Close button to close the Print Preview
window.
Or
1Choose the Print button to send the page or pages to
the output device, using the defaults set in the Print
Setup dialog box.
capug.book Page 99 Tuesday, May 23, 2000 12:08 PM
Chapter 5 Printing and plotting
100
Scaling printer or plotter output
You can manually scale, or have Capture automatically
scale, printer output and plots to fit a given paper size.
To scale a print or a plot
1From the File menu, choose Print. The Print dialog box
appears.
2Select one of the three options in the Scale box.
The Scale to paper size option scales each
schematic page to fit a single sheet of paper (as
configured in the printer driver).
The Scale to page size option scales each schematic
page to the sheet size you select in the Page size
area. The sheet size is configured in the Page Size
tab in the Design Template dialog box.
The Scaling option scales your schematic page to a
factor between 0.100 and 10.000.
3If you select the Scale to page size option in step 2, the
Page size area becomes available. Select a sheet size.
This results in multiple sheets of paper if you select a
sheet size larger than your printer paper.
4Click OK to print the image.
capug.book Page 100 Tuesday, May 23, 2000 12:08 PM
Special considerations for plotting
101
Special considerations for
plotting
Vector (pen) plotters do not support bitmaps directly. If
you are sending Capture output to such a plotter, it will
not plot your bitmaps. Most inkjet and thermal plotters
will plot bitmaps.
Plotter pen colors
The plotter driver maps your color choice to the closest
available pen color as established in your plotter driver
configuration. See your plotters driver setup and
documentation for more details.
Many plotters do not have drivers that ship with
Windows. If you do not see the plotter you are looking for
in the list of available drivers, contact your plotter
manufacturer and ask for a Windows driver. If your
plotter emulates HPGL, use the HPGL driver as an
alternative solution.
T
ip Vector-based plotters tend to produce
higher quality output than raster-based
printers.
Note The plotter setup dialog boxes are
only accessible from the Windows Control
Panel. See the documentation included with
Microsoft Windows regarding the Windows
Control Panel.
capug.book Page 101 Tuesday, May 23, 2000 12:08 PM
Chapter 5 Printing and plotting
102
capug.book Page 102 Tuesday, May 23, 2000 12:08 PM
Part Two
Creating designs
Chapter 6, Design structure, describes how to customize the
working environment specific to your system, how to
create default settings for new designs, and how to
override default settings in individual designs.
Chapter 7, Placing, editing, and connecting parts and symbols,
describes how to place and edit parts and symbols. It also
describes how to connect the elements of your design
using hierarchical blocks, hierarchical ports, off-page
connectors, wires, and buses.
Chapter 8, Adding and editing graphics and text, describes the
drawing tools you can use to add text and a variety of
graphic shapes to your design.
Chapter 9, Using macros, describes how to create and run
macros.
Chapter 10, Changing your view of a schematic page,
describes how to view specific areas of a schematic page
using the Zoom command. It also describes jumping to
different locations within a schematic using the Location,
Reference, and Bookmark commands.
capug.book Page 103 Tuesday, May 23, 2000 12:08 PM
capug.book Page 104 Tuesday, May 23, 2000 12:08 PM
Design structure
6
Many schematic designs can fit on one schematic page.
Some designs, however, are too large for even the biggest
page, and even if a complex design could fit on one page,
there are good reasons for dividing it:
To fit at full scale on your printers page.
To partition a design so that several people can work
on it at once.
To develop the design using a top-down approach.
That is, you may want to begin with a block diagram
in which each block represents a major function and
then construct more detailed diagrams for each block.
To organize your design by functional parts.
To meet department specifications.
Capture offers two ways of handling multiple-page
designs: a flat design structure and a hierarchical design
structure.
capug.book Page 105 Tuesday, May 23, 2000 12:08 PM
Chapter 6 Design structure
106
Flat designs
Flat designs are practical for small designs with few
schematic pages. A flat design is a structure in which the
output nets of one schematic page connect laterally to the
input nets of another schematic page in the same
schematic folder through objects called off-page connectors.
A flat design has no hierarchy (no hierarchical blocks,
hierarchical ports, hierarchical pins, or parts with attached
schematic folders). The structure of a flat design is shown
to the left.
All schematic pages in a flat design are contained within a
single schematic folder, and are on a single level, as shown
at left. In the figure, SCHEMATIC1 is a schematic folder.
It contains schematic pages named PAGE1 and PAGE2.
Since you must manage all of the interconnections
between the pages of a flat design using names assigned
to off-page connectors, it is best to keep a flat design
relatively small.
capug.book Page 106 Tuesday, May 23, 2000 12:08 PM
Hierarchical designs
107
Hierarchical designs
You can create symbols on schematic pages that represent
other schematic folders. These symbols are called
hierarchical blocks. The layered arrangement created by
placing schematic folders inside schematic pages is called
a hierarchy.
Any schematic page can contain hierarchical blocks (or
parts with attached schematic folders) that refer to other
schematic folders; a designs structure can be many levels
deep. The schematic folder at the top of a hierarchy, which
directly or indirectly refers to all other schematic folders
in the project, is called the root module.
In the project manager, the root module has a backslash in
its folder icon. The root module, as well as any other
schematic folder, can contain as many schematic pages as
you need.
Simple hierarchical designs
Figure 34 An abstract representation of a simple hierarchy.
T
ip If you intend to take your design into
a digital simulator like PSpice, it is best to
place only one schematic page in each
lower level schematic folder. This may
reduce problems you encounter while
troubleshooting your designs.
Schematic A
Schematic B Schematic C
Schematic D Schematic E Schematic F
capug.book Page 107 Tuesday, May 23, 2000 12:08 PM
Chapter 6 Design structure
108
A one-to-one correspondence between hierarchical blocks
(or parts with attached schematic folders) and the
schematic folders they reference is called a simple hierarchy
(Figure 35).
In a simple hierarchy, each hierarchical block or part with
an attached schematic folder represents a unique
schematic folder.
Figure 35 A simple hierarchical design, as
seen in the project manager
capug.book Page 108 Tuesday, May 23, 2000 12:08 PM
Hierarchical designs
109
Complex hierarchies
A many-to-one correspondence between hierarchical
blocks (or parts with attached schematic folders) and the
schematic folders they reference is called a complex
hierarchy. In Figure 36, schematic A references schematic B
three different times. These references can be via
hierarchical blocks or parts with attached schematic
folders.
Figure 37 shows a complex hierarchical design as seen on
the Hierarchy tab of the Capture project manager. Figure 36 An abstract representation of a
complex hierarchy
Schematic A
Schematic B
Figure 37 A complex hierarchical design,
as seen in the project manager
capug.book Page 109 Tuesday, May 23, 2000 12:08 PM
Chapter 6 Design structure
110
Connecting schematic folders and
schematic pages
In Capture, you connect schematic folders and schematic
pages by extending nets between them using hierarchical
blocks (or parts with attached schematic folders),
hierarchical ports, hierarchical pins, and off-page
connectors. Hierarchical blocks (or parts with attached
schematic folders), hierarchical ports, and hierarchical
pins carry signals between schematic folders and
schematic pages in a hierarchy, while off-page connectors
carry signals between schematic pages within a single
schematic folder of a flat design.
Hierarchical blocks
Hierarchical blocks (or parts with attached schematic
folders) refer to child schematics in a design, providing
vertical (downward-pointing) connection only.
Hierarchical pins in a hierarchical block, and hierarchical
ports outside a hierarchical block, act as points of
attachment for electrical connections between the
hierarchical block and other electrical objects in an
attached schematic folder. The picture at left shows
hierarchical pins (X, Y, SUM, and CARRY) within a
hierarchical block, and a hierarchical port (CARRY_IN)
outside a hierarchical block.
A part with an attached schematic folder functions like a
hierarchical block, and pins on a part with an attached
schematic folder function like hierarchical pins within a
hierarchical block. You can use either method to define a
hierarchy. The only difference between the methods is
that a part with an attached schematic folder can be
reused.
For information about placing hierarchical
blocks, hierarchical ports, hierarchical pins,
and off-page connectors, see Chapter 7,
Placing, editing, and connecting parts and
symbols.
Note Before you create or resize a
hierarchical block, make sure the Snap to
g
rid option is turned on (by choosing
Preferences from the Options menu). If the
hierarchical block is off grid, then
hierarchical pins inside it are also off
g
rideven if you change the Snap to grid
setting before you place themand it
may be difficult to connect to these off-grid
hierarchical pins.
capug.book Page 110 Tuesday, May 23, 2000 12:08 PM
Connecting schematic folders and schematic pages
111
You can attach a schematic folder that is external to a
project to a hierarchical block, but be aware that you wont
be able to use any of Captures tools to make changes to
the external design unless you explicitly open that
external design.
Caution If you incorporate an external schematic folder into a hierarchical
block, include the schematic folder when you give the project to
another engineer or to a board fabrication house. Attached
schematic folders external to a project do not automatically
accompany schematic folders that you copy or move to another
project. For this reason, you should copy all attached schematic
folders into your project if you want your project to be portable.
Hierarchical ports
Hierarchical ports provide vertical (upward-connecting)
and lateral connections within a design hierarchy. A
hierarchical port connects vertically to a like-named
hierarchical pin inside a hierarchical block, and connects
laterally to like-named nets in the same schematic page,
and hierarchical ports within the same schematic folder.
Hierarchical pins
Hierarchical pins provide vertical (downward-pointing)
connections only. You connect them by name to
hierarchical ports on schematic pages in an attached
schematic folder. Think of hierarchical pins as bringing a
net up from an attached schematic folder into the
hierarchical block, but not out onto the schematic page. In
the figure shown, X, Y, SUM and CARRY represent
hierarchical pins.
capug.book Page 111 Tuesday, May 23, 2000 12:08 PM
Chapter 6 Design structure
112
Off-page connectors
Off-page connectors provide connection between
schematic pages within the same schematic folder. An
off-page connector is connected by name to other off-page
connectors within the same schematic folder. Like-named
off-page connectors in different schematic folders are not
connected.
capug.book Page 112 Tuesday, May 23, 2000 12:08 PM
An example: creating a simple hierarchy
113
An example: creating a simple
hierarchy
As described earlier in this chapter, you connect schematic
folders and schematic pages by extending nets between
them using off-page connectors, hierarchical ports, and
hierarchical pins in hierarchical blocks. Off-page
connectors carry nets between schematic pages within a
single schematic folder. Hierarchical blocks, hierarchical
ports, and hierarchical pins carry nets between schematic
folders, which need not be in the same design.
The rest of this section contains an example of how to use
off-page connectors, hierarchical ports, hierarchical pins,
and hierarchical blocks to create a simple hierarchy.
Figure 38 shows two schematic folders (Sch. A and
Sch. B), each with two schematic pages. The schematic
folder marked with a backslash (\) is called the root
module.
To establish a hierarchy with schematic folder A positioned
above schematic folder B
Figure 39 illustrates the schematics with hierarchy
established.
1Place a hierarchical block on schematic page 1.
2In the Place Hierarchical Block dialog box, set the
following options to attach schematic folder B:
Type in a reference.
Select Schematic View for the Implementation
Type.
Type in Sch.B as the Implementation Name.
Note For information about placing
hierarchical blocks, hierarchical ports,
hierarchical pins, and off-page connectors,
see Chapter 7, Placing, editing, and
connecting parts and symbols.
Figure 38 Schematics before hierarchy
Figure 39 Schematics with hierarchy
capug.book Page 113 Tuesday, May 23, 2000 12:08 PM
Chapter 6 Design structure
114
To carry a net between schematic folder A and schematic folder B
Figure 40 illustrates the schematics carrying a net between
them.
1Select the hierarchical block on schematic page 1 and
place a hierarchical pin named X inside it.
The hierarchical pin is a point of attachment for
electrical connections between the hierarchical block
and other objects on schematic page 1.
2Place a hierarchical port named X on schematic
page 3.
The hierarchical port is a point of attachment for
electrical connections between schematic page 3 and
other schematic pages within schematic folder B. It is
connected by name to the hierarchical pin inside the
hierarchical block on schematic page 1.
Hierarchical ports generally carry a net up through a
hierarchy. In a root module, they usually represent
external signals, such as a hierarchical block in another
project.
The two hierarchical ports added to schematic folder A
are electrically connected to each other by the name Y,
so any electrical objects (such as power or ground
symbols) on schematic pages 1 and 2 named Y are part
of the net named Y. You could make both of these
hierarchical ports off-page connectors without affecting
the electrical connections. Figure 41 illustrates this
electrical connectivity across pages in a schematic.
To connect the schematic pages in schematic folder B,
place a hierarchical port named X on schematic page 4.
Any like-named electrical objects on schematic pages 3
and 4 are now part of a single net named X.
To connect the X nets in schematic folder B and the Y
nets in schematic folder A, you cannot simply rename one
set of objects to match the other set of objects. Remember,
the hierarchical pin X inside the hierarchical block on
schematic page 1 does not bring net X out onto
schematic page 1. You must physically connect
hierarchical pin X to net Y in order to join the two
nets.
Figure 40 Schematics carrying a net
Figure 41 Connectivity across pages in a
schematic
capug.book Page 114 Tuesday, May 23, 2000 12:08 PM
Placing, editing, and
connecting parts and symbols
7
Capture includes libraries containing parts, power
symbols, and ground symbols. You can place instances of
these objects on a schematic page. Once you place a part,
you can edit its appearance, properties, or location. Once
you have placed a power or ground symbol, you can
rotate it or edit its name.
This chapter contains information about placing and
editing objects from Capture libraries. It also explains how
to connect these objects using wires and buses.
Figure 42 Schematic with power and ground symbols
capug.book Page 115 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
116
Capture libraries also include symbols used to establish
connectivity between schematic pages. You use off-page
connectors to connect signals between schematic pages
within a schematic folder. You use hierarchical blocks,
hierarchical ports, and hierarchical pins to connect signals
from one schematic folder to another, or from an attached
schematic folder. See An example: creating a simple hierarchy
on page 113 for more information on working with
connectivity across schematic pages.
Wires and buses are used to conduct signals between
parts and electrical objects. Nets are made up of one or
more wires; a bus represents multiple signals or nets.
capug.book Page 116 Tuesday, May 23, 2000 12:08 PM
Placing and editing parts
117
Placing and editing parts
Capture includes libraries with a total of over 30,000 parts
that you can use on your schematic pages. You can also
create your own parts.
A library part has a package view, which corresponds to
the actual physical object that can be placed, for example,
on a printed circuit board. The package view identifies the
physical pin numbers and the number of logical objects
(for example, parts or devices) that are contained within
the package.
Figure 43 Part editor in package view
The different parts that make up a package can be
identical in their graphic appearance and electrical
connectivity (homogeneous) or they can be dissimilar in
their graphic appearance or electrical connectivity
(heterogeneous).
In addition to the package view, a library part has a part
view, which is a graphical representation used to define a
single, logical, electrical object whose electrical
connectivity is represented by pins.
Note For information about creating your
own parts, see Chapter 12, Creating and
editing parts.
capug.book Page 117 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
118
Figure 44 Part editor in part view
Each part has a set of properties that contains
informationsuch as part value and reference
designatorused by layout or simulation tools. In
addition, you can create your own unique part properties
that hold information relevant to your application.
Parts have pins that define the parts electrical
connectivity. Pins carry information in properties that
define the characteristics of each pin. This information
includes the pins name, number, shape (clock, dot,
dot-clock, line, short, or zero length), type (3-state,
bidirectional, input, open collector, open emitter, output,
passive, or power), width (scalar or bus), and visibility.
The pin type is used by the Design Rules Check command
on the Tools menu to check conformance to basic electrical
rules.
A primitive part is a basic part without any underlying
hierarchy. A nonprimitive part is a part that has an
underlying hierarchy, such as an attached schematic
folder, PSpice model, or VHDL code. Placing a
nonprimitive part adds all its underlying hierarchy to
your project without moving the actual schematic folders,
making it easy to add levels of hierarchy to your project.
Placing parts
You select parts from libraries and place them on
schematic pages using the Part command on the Place
T
ip A part doesnt necessarily need pins. If
a part doesnt have pins, it is listed in a bill
of materials report, but doesnt appear in a
netlist. This is useful if you want to show
hardwaresuch as screws, nuts, or
w
ashersin a bill of materials report.
Note A part without pins will not snap to
g
rid when placed on a schematic page.
capug.book Page 118 Tuesday, May 23, 2000 12:08 PM
Placing and editing parts
119
menu, or using the part tool on the schematic page editor
tool palette.
Alternatively, if youve placed the part or symbol recently,
place the part using the Most Recently Used (MRU) list on
the Capture toolbar. See To place a part using the Most
Recently Used (MRU) List on page 7-120.
To place a part
1From the schematic page editors Place menu, choose
Part.
or
Choose the part tool on the schematic page editors
tool palette.
The Place Part dialog box appears.
2Select a part from the list that appears.
or
In the Part text box, type the name of the part. If you
arent sure of the name of the part, enter wildcard
characters to constrain the list of parts, then click OK.
Valid wildcard characters are an asterisk (*) to match
multiple characters and a question mark (?) to match a
single character.
After you type the name of the part to be placed, click
OK. All parts in the libraries (listed in the Libraries list
box) that match the part name appear in the box below
the Part text box. When you select a part from this box,
its graphic image displays in the preview box.
3When you have located the part you want to place,
click OK.
An image of the selected part is attached to your
pointer. You can click the right mouse button to
display a pop-up menu with commands that you can
use to change the properties of the part before you
place it. You can mirror the part horizontally or
vertically, rotate the part, or edit the parts properties.
4Move the pointer to the location on your schematic
page where you want to place the part, then click the
left mouse button.
T
ip You can add more libraries to the
Libraries list box by clicking Add Library.
T
ip You can remove a library from the
Libraries list box by selecting it and clicking
Remove Library.
T
ip You can switch to the convert view of a
part while placing it using the Graphic
option on the Place Part dialog box.
T
ip If your part is a multiple-part package,
y
ou can select which part in the package to
view using the Part drop-down list in the
Packaging area of the Place Part dialog
box.
Note All schematic page objects have right
mouse button pop-up menus. These menus
are context sensitive, displaying commands
appropriate for the selected object. For
information about pop-up menu
commands, see the Capture online help.
capug.book Page 119 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
120
This places an instance of the part on your schematic
page. (You can place multiple instances of the part by
clicking the left mouse button at each location where
you want an instance of the part.)
5When you are done placing instances of the selected
part, choose End Mode from the right mouse button
pop-up menu, or press E.
To place a part using the Most Recently Used (MRU) List
1While the schematic page editor is active, select a part
or symbol from the MRU list on the Capture toolbar.
An image of the selected part is attached to your
pointer. You can click the right mouse button to
display a pop-up menu with commands that you can
use to change the properties of the part before you
place it. You can mirror the part horizontally or
vertically, rotate the part, or edit the parts properties.
2Move the pointer to the location on your schematic
page where you want to place the part, then click the
left mouse button.
This places an instance of the part on your schematic
page. (You can place multiple instances of the part by
clicking the left mouse button at each location where
you want an instance of the part.)
3When you are done placing instances of the selected
part, choose End Mode from the right mouse button
pop-up menu, or press E.
Note To select a part, point-and-click, type
into the list box, or press C+M. For
information about the MRU list, see Most
Recently Used (MRU) part list on page
124.
Note All schematic page objects have right
mouse button pop-up menus. These menus
are context sensitive, displaying commands
appropriate for the selected object. For
information about pop-up menu
commands, see the Capture online help.
capug.book Page 120 Tuesday, May 23, 2000 12:08 PM
Placing and editing parts
121
Place Part dialog box
Figure 45 Place Part dialog box
Part Specifies the name of the part. Start typing the part
name and if Capture finds the part in the selected libraries,
it will automatically complete the part name for you.
If you arent sure of the exact name of the part, you can
enter wildcard characters to constrain the list of parts,
then click OK. Valid wildcard characters are an asterisk (*)
to match multiple characters and a question mark (?) to
match a single character. The names of all parts in the
selected libraries that match the wildcard appear in the
Part list box.
capug.book Page 121 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
122
Part list Lists the names of all parts in the selected
libraries that match the name entered in the Part text box.
If more than one library is selected, the part name is
followed by a forward slash (/) and a library name. When
you select a part in the list, its name appears in the Part
text box, and its graphic displays in the preview box.
The full path of the library appears when you hover your
pointer over a part or a library name in the part list.
Libraries Lists the library names currently available.
All parts in the selected libraries that match the Part text
box appear in the Part list. To select more than one library,
hold C while you click the mouse. To select all the
libraries in the list, press C+a.
The full path of the library appears when you hover your
pointer over the library name.
Graphic You can choose the view of the part: Normal or
Convert. Some parts have a Convert view that is used for
things such as a DeMorgan equivalent of a part.
Packaging Parts per package indicates the number of
parts in the package you are editing. Part indicates which
part of a multiple-part package you are placing.
Preview box Displays the graphic of the selected part.
Application Indicator Four possible property values
(Layout, Schematic View, VHDL, and PSpice) cause one
or more icons to appear at the bottom of the Place Part
dialog box while you place a part that has one or more of
the properties. A schematic view or VHDL
implementation type property causes the Schematic View
or VHDL icon to appear, while the PSpice icon indicates
that a PSpice Template property exists and the Layout
icon shows that a PCB Footprint property is on the part or
symbol. The name of the relevant downstream tool
appears when you hover your pointer over the icon.
capug.book Page 122 Tuesday, May 23, 2000 12:08 PM
Placing and editing parts
123
Add Library Displays a standard Open dialog box that
you can use to locate a library and add it to the Libraries
Remove Library Removes the selected libraries from
the Libraries list.
Part Search Opens the Part Search dialog box, so you
can search for a part in all the libraries listed in a particular
directory.
Note If you select an SDT 386+ or SDT
Release IV library from the dialog box that
appears when you choose Add Library,
Capture automatically translates the file
after you specify the name of the new
Capture library.
capug.book Page 123 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
124
Most Recently Used (MRU) part list
The Most Recently Used list is in the middle of the
Capture toolbar. It is enabled only the window of a
schematic page is active.
Each time you place a part or symbol using a command
from the Place menu, the name of that same part or
symbol is added to the top of the MRU list. When you
select a part or symbol from the MRU list and use it in
your design, the name of that item moves to the top of the
list.
The MRU list holds up to 25 placed items for a given
project. If you exceed that limit, Capture removes the last
part or symbol from the list and places the name of the
most recently placed item at the top of the list.
Capture saves the MRU list on a project-by-project basis
for each session. If you have more than one project open,
the list updates for the active project.
You can select a part from the MRU list using any of these
methods:
Use the mouse. Expand the MRU drop-down list by
clicking on the arrow at the right of the list, then click
on a part or symbol to select it.
Type the part or symbol name. Click in the MRU list
box and begin typing the name of the part or symbol.
Capture automatically completes the name if the item
is in the list. When the name is highlighted in the MRU
list box, press R.
If the part or symbol is not in the MRU list, but is a part
in the set of configured libraries, an image of the part
attaches to your pointer when you press R.
Use the shortcut. Press C+M to highlight a part in
the MRU list. Press t and b to select a part or
symbol in the list. When the correct part or symbol is
highlighted in the list box, press R.
capug.book Page 124 Tuesday, May 23, 2000 12:08 PM
Placing and editing parts
125
Searching for parts
Capture can search for a particular part inside all the
libraries it finds in the specified directory.
To find a part
1In the schematic page editor, choose Part from the
Place menu.
2Click the Part Search button. The Part Search dialog
box appears.
3Enter the part name you want to locate.
4Click Browse to locate the directory where your
libraries are located.
5Click Begin Search. Capture returns the names of all
the libraries in the specified directory, that contain
your part.
Editing parts
You can move a part on a schematic page by selecting it
and dragging it to a new location. You can use the Rotate
or the Mirror command from the Edit menu. You can use
the part editor to change the parts physical appearance,
and you can edit the parts properties. When you edit a
part on a schematic page, your edited part differs from the
part in the library and exists only in your design; you can
place another copy of the part you edited by using the
Copy command from the Edit menu, and by dragging the
part from the design cache.
Note Using the Find command on the
schematic page editors Edit menu, you can
specify a search and replace for parts, nets,
title blocks, off-page connectors, flat nets,
power or ground symbols, bookmarks,
hierarchical ports, text, or DRC markers.
Note For more information about editing
parts, see Chapter 12, Creating and editing
parts.
capug.book Page 125 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
126
To edit the physical appearance of a part, select it, and
either choose Part from the Edit menu or choose Edit Part
from the right mouse button pop-up menu. This opens the
part in a part editor window. After you finish editing the
part and choose Save, youre given a choice of updating
the single instance, or updating all instances in the design.
If you update only the single instance, Capture creates a
new part in the design cache. If you update all instances,
Capture replaces the library part in the design cache with
your edited part. These new parts are placed in the design
cache with -n appended to the name, where n is an
integer.
To edit the properties of a part, select the part on the
schematic page, and either choose Properties from the
Edit menu, or choose Edit Properties from the right mouse
button pop-up menu. You can also double-click the part.
This displays the property editor, shown in Figure 46.
Figure 46 Property editor with filter set to Capture
Capture displays properties according to the selected
filter. All the properties are shown when the filter is set to
All. General schematic page properties are shown when
the filter is set to Capture. The following are common
properties:
Value Specifies the part value name. By default, the part
value is set to the name of the part if you dont specify a
part value in the library.
capug.book Page 126 Tuesday, May 23, 2000 12:08 PM
Placing and editing parts
127
Reference Specifies the part reference.
Primitive Default indicates that the part uses the
setting in the Hierarchy tab of the Design Properties
dialog box. Yes indicates that the part is primitive. No
indicates that the part is nonprimitive.
Designator Indicates which part of a multiple-part
package you are editing.
PCB Footprint The PCB physical package name to be
included for this part in the netlist.
Power Pins Visible Specifies the visibility of the parts
power pins.
Implementation Type Specifies if the part has an
attached schematic folder or other implementation, and
the type of implementation, if one exists. Implementation
types include schematic folders, VHDL entities, netlists,
and PSpice models.
Caution An attached schematic folder or other file external to the project or
library is not stored with the project or library. If you copy or move
the project or library to a new location, you must also move or copy
the attached object to keep them together. In addition, you may
need to edit the path to the attached schematic folder or file if you
move the project to a new location with a different directory
structure.
N
ote
T
o c
h
ange t
h
e
P
art
R
e
f
erence
property, you will need to edit the
Reference property, the Designation
property, or both. The Part Reference
property is a read-only property that
Capture calculates from the Reference and
Designator values.
Note For information on power pin
visibility and how it affects a global net, see
the Capture online help.
capug.book Page 127 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
128
Placing and editing power and
ground symbols
You can place power and ground symbols, and you can
edit their names before or after placing them. You can also
edit the text associated with the symbols. The name of a
power symbol becomes the name of the global net that is
created.
Placing power and ground symbols
Power and ground symbols are placed on a schematic
page using the Power command or Ground command on
the Place menu, or using the power tool or ground tool on
the tool palette. Power and ground symbols are selected
from libraries the same way parts are selected from
libraries. CAPSYM.OLB contains all the power and
ground symbols shipped with Capture.
To place a power symbol
1From the schematic page editors Place menu, choose
Power.
or
Choose the power tool on the schematic page editors
tool palette.
The Place Power dialog box appears.
2In the Symbol text box, type the name of the symbol to
place. If you arent sure of the exact name of the
symbol, you can enter wildcard characters to constrain
the list of symbols, then press R. Valid wildcard
characters are an asterisk (*) to match multiple
characters and a question mark (?) to match a single
character. All power symbols in the libraries selected
in the Libraries list box that match the name of the
power symbol are listed in the box below the Power
Symbol text box. When you select a symbol from this
box, its graphic image appears.
Figure 47 Power and ground symbols in
CAPSYM.OLB
capug.book Page 128 Tuesday, May 23, 2000 12:08 PM
Placing and editing power and ground symbols
129
3After you locate the power symbol you want to place,
click OK. An image of the power symbol is attached to
your pointer.
You can press the right mouse button to display a
pop-up menu with commands to change the attributes
of the power symbol before you place it. You can
mirror the power symbol horizontally or vertically, or
rotate it.
4Move the pointer to the location on your schematic
page where you want the power symbol and click the
left mouse button. This places the power symbol on
your schematic page.
You can place multiple instances of the power symbol
by clicking the left mouse button each place you want
an instance of the symbol.
5When you are done placing power symbols, choose
End Mode from the right mouse button pop-up menu,
or press E.
To place a ground symbol
1Follow the instructions in the previous section, To
place a power symbol on page 7-128, but substitute the
Ground command or the ground tool in the
appropriate places.
Note All objects that you can place on a
schematic page have right mouse button
pop-up menus. These menus are context
sensitive, meaning they display commands
that are appropriate for the selected object.
For information about the commands on a
pop-up menu, see Captures online help.
Note You can create custom power,
g
round, and other symbols for hierarchical
ports, off-page connectors, title blocks, and
power objects by choosing the New Symbol
command from the Design menu in the
project manager window. For information
on how to use this command, see Captures
online help.
capug.book Page 129 Tuesday, May 23, 2000 12:08 PM
Chapter 7 Placing, editing, and connecting parts and symbols
130
Place Power and Place Ground dialog boxes
The Place Power and Place Ground dialog boxes are
identical, except that each displays the last power or
ground symbol you placed on this page. This figure shows
the Place Power dialog box.
Figure 48 Place Power dialog box
Symbol Specifies the name of the power or ground
symbol in the library. If you arent sure of the exact name
of the symbol, you can enter wildcard characters to
constrain the list of symbols, then click OK. Valid
wildcard characters are an asterisk (*) to match multiple
characters and a question mark (?) to match a single
character. The names of all symbols in the selected
libraries that match the wildcard appear in the Symbol list
box.
Symbol list Lists the names of all symbols in the
selected libraries that match the name entered in the
Symbol text box. If more than one library is selected, the
symbol name is followed by a slash (/) and a library name.
When you select a symbol in this list, its name displays in
the Symbol text box, and its graphic displays in the
preview box.
capug.book Page 130 Tuesday, May 23, 2000 12:08 PM
Placing and editing power and ground symbols
131
Libraries Lists the library names currently available.
Select the libraries from which to select power or ground
symbols. All symbols in the selected libraries that match
the Symbol text box display in the Symbol list. To select
more than one library, press C while you click the
mouse.
Preview box Displays the graphic of the selected
symbol.
Add Library Displays a standard Open dialog box that
you can use to locate a library and add it to the Libraries
list.
Remove Library Removes the selected libraries from
the Libraries list.
Name Assigns a namesuch as +5, GND, +5VDC, -12
VDC, VSS, or VEEto the symbol. By default, the name of
the symbol is assigned.
Editing power and ground symbols
You can change the name of a power or ground symbol by
selecting the symbol on the schematic page, and either
choosing Properties from the Edit menu, or choosing Edit
Properties from the right mouse button pop-up menu.
You can also double-click the symbol. This displays a
dialog box in which you can edit the symbols name, then
click OK.
You can also edit the display properties of the name of the
power or ground symbol. Select only the text of the
symbol, then either choose Properties from the Edit menu,
or choose Edit Properties from the right mouse button
pop-up menu. You can also double-click the text. This