Orcad Capture User Guide

Orcad® Capture

User’s Guide

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

Cadence PCB Systems Division 13221 SW 68th Parkway, Su ite 200 Portland, OR 97223

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

Contents

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

Contents

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 Orcad’s 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

Contents

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

Contents

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

vii

Contents

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 part’s convert . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239

Part Four Processing your design

About the processing tools 243Chapter 13

Tools overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 244

viii

Contents

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

Contents

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

Figures

Figure 1 Capture’s 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 Programmer’s editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

Figure 8 Session log . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14

Figure 9 Capture’s 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

Figures

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

xii

Figures

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

xiii

Figures

xiv

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 Capture’s 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

Tables May 22, 2000

xvi

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 ci rcuit board layout. What’s more, Orcad family products are a suite of applications built around an engineer's design flow—not just a collection of independently developed point tools. 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 C apture’s tools to quickly annotate it and prepare it for the next stage of development.

Before you begin

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; gene rating 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+r Press C+r. Means to hold down the C key while

pressing r.

A, f, o From the File menu, choose Open (A, f,

o).

xviii

Means that you have two options. You can use the mouse to choose the Open command from the File me nu, or you can press each of the keys in parentheses in order: first A, then f, then o.

How to use this guide

Monospace font

UPPERCASE In Capture, open CLIPPERA.DSN. Path and filenames are shown in

Italics In Capture, save design_name.DSN. Information that you are to provide is

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 the example, you open the design file named CLIPPERA.DSN.

shown in italics. In the example, you save the design with a name of your choice, but it must have an extension of .DSN.

Getting started

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

1 From the Start menu, point to Programs and choose

Orcad Family Release.

2 From the Orcad Family Release menu item, choose

Capture.

Chapter 1 Getting started

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 Capture’s session frame

The minimized Session Log icon in the lower left portion of the Capture session frame is the sessi on log. The session log provides information about everything you have done in the current Capture session. Detailed information about this window—and the other windows in Capture—is given in Chapter 2,

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 avail able me nus and menu choices also vary depending upon the type of project.

The Capture work environment.

The Capture work environment

This chapter describes the things you need to know to find your way around in Capture. It shows the windows you’ll 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.

Chapter 2 The Capture work environment

Figure 2 New project manager window

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 doesn’t actually contain all the resources. It merely “points to” the various files that the project uses. For this reason, be sure you don’t move or delete any f iles referenced by a project. If you do, the project won’t 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

For information a bout hierarch ical designs , see Chapter 6,

Design structure.

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 design’s 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.

• The Library folder (in the Design Resources folder)

shows the schematic part library files you’ve add ed to the project using the Project command on the Edit menu.

• The Outputs folder shows the output of Capture’s

processing tools. Generally, these files include bill of materials reports and technology-specific netlists. Capture adds files to this folder when each is created.

The project manager

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 c ontents are vis ible, liste d below the folder. It appears as a schematic f older 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

C key while you drag them. If you close a project

the manager window, you close the project.

ip The root module for a design has a

backslash in its folder icon, as shown in Figure2 on page 2-6.

Note If a schematic page is open, you

cannot drag its icon to a different location.

In the project manager’s 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.

Chapter 2 The Capture work environment

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 fo lders. A s chemati c 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.

Note The project manager is also used to

manage libraries and the parts they contain. This is covered in detail in Chapter11, About libraries and parts.

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 manager’s Edit menu, the Print command on the project manager’s File menu, and the various tools on the Tools menu only apply to the selected schematic folder or page.

Project manager tabs—File and Hierarchy

The project manager provides two ways to display a project’s resources.

If you choose the File tab (shown in Figure 3), the project manager displays all the project’s 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 project’s schematic folders and schematic pages.

For information abou t simple and complex hi erarchical designs, see Chapter 6,

Design structure.

The project manager

Figure 3 File tab

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 4 Hierarchy tab

Chapter 2 The Capture work environment

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 ava ilable 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.

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 f rom within the schematic page editor, or from the project manager window.

The schematic page editor

Figure 5 Schematic page editor

Chapter 2 The Capture work environment

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.

For more information, see The part

editor tool palette on page 2-22.

See Chapter 11,

and parts for complete definitions of

parts and packages. See Chapter 12,

Creating and editing parts for a

complete description of the part editor.

About libraries

• Use the tool palette’s 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 editor’s lack of Pin and Pin Array tool palette buttons.

The programmer’s editor

Use the programmer’s 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 Programmer’s editor

To create a new VHDL file in the programmer’s editor

1 From the File menu, point to New, then choose VHDL

File. A blank VHDL file appears in the text editor.

The programmer’s ed itor

To open a VHDL file in the programmer’s editor

1 From the File menu, point to Open, then choose VHDL

File. The Open VHDL File dialog box appears.

2 Select a file, then click OK.

1 In the project manager, select a VHDL file. 2 Click the right mouse button, and choose Edit from the

pop-up menu.

oteDesigns and parts of designs can be

VHDL-based instead of schematic-based.

Chapter 2 The Capture work environment

TipY

The session log

The session log lists the events that have occurred during the current Capture session, including messages resulting from using Capture’s tools. To display context-sensitive help for an error message, put the cursor in the error message line in the session log and press

The ruler along the top appears in either inches or millimeters, depending on which measurement system (U.S. or Metric) you have select ed 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.

ou can clear the session log by choosing the Clear Session Log co mma nd , or by pressing

C+ X.

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 u seful when working with Orcad’s customer support staff to solve technical problems. The default filename is SESSION.TXT.

To display the session log

1 Click on the session log’s maximize button, or choose

Session Log from the Window menu.

To minimize the session log

1 Click the minimize button on the title bar.

To copy session log text to th e Clipboard

1 Select the session log window to make it active. 2 Select the text and choose Copy from the Edit menu.

To print the session log

1 Select the session log window to make it active. 2 From the File menu, choose the Print command.

To use Find in the session log

1 Select the session log window to make it active.

The session log

2 From the Edit menu, choose the Find command. The

Find dialog box appears.

3 Enter the word or words that you want to find. 4 Click Find Next.

To save the session log to a text file

1 Select the session log window to make it active. 2 From the File menu, choose the Save As command.

The Save As dialog box appears.

3 Enter a file name in the File name text box. By def ault,

the session log is saved to SESSION.TXT in the current directory. If necessary, specify a new location for the file.

4 Click Save. The session log text is saved to the file.

Chapter 2 The Capture work environment

The toolbar

oteThe toolbar is always docked on the

top edge of the session frame the first time

ou open a project in a new session frame of Capture. The position of the tool palet t e is not saved.

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

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

designs, libraries, and VHDL files on page 3-55.

Capture’s 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 can’t perform that task in the current situation.

Figure 9 Capture’s 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.

Creating

Opening existing projects,

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

Cut Remove the selected object and place it on the Clipboard. Eq uivalent 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.

Chapter 5, Printing and plotting.

Table 1 Tools on the Capture toolbar (continued)

Paste Paste the contents of the Clipboard at the cursor. Equivalent to the

Paste command on the Ed i t me n u.

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

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

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

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

The toolbar

To place a part using the Most

To zoom in on

To zoom ou t

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 selecte d schematic pages.

Equivalent to the Annotate command on the Tools menu. For more information, see

Back Annotate Back annotate the selected schematic pages. Equivalent to the Back

Annotate command on the Tools menu. For more information, see

Annotating on page 14-247 .

Back annotating on page14-266.

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.

Chapter 2 The Capture work environment

Table 1 Tools on the Capture toolbar (continued)

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

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

Snap-to-Grid Toggle schematic page and part editing to ei ther on or off grid.

Project Manager Di splay 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.

Creating a cross reference report on

Creating a bill of materials on page 16-275.

Displaying or hiding the toolbar

You can hide the toolbar, then display it again when you need it.

To display or hide th e toolbar

1 From the schematic page editor’s View menu, choose

Toolbar.

From the part editor’s View menu, choose Toolbar.

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 tool’s 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.

The tool palet te s

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.

Figure 10 Schematic page editor tool palette

Table 2 describes the tools on the schematic page editor tool palette.

For information on using the electrical tools, see Chapter 7,

editing, and conne cting parts and symbols. For information on how to use

the drawing tools, see Chapter 8,

Adding and editing graphic s and

Placing,

Chapter 2 The Capture work environment

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

non-orthogonal (not a multiple of 90°) wires. Equivalent to the Wire command on the Place menu. For more information, see

S to draw

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

Bus Draw buses. Press S to draw

non-orthogonal segments. Equivalent to the Bus command on the Place menu. For more information, see

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 buses on page 7-152.

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 symbo l s. Equivalent to the Ground

command on the Place menu. For more information, see

Placing power and ground

symbols on page 7-128.

Table 2 Tools on the schematic page editor tool palette (continued)

The tool palet te s

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 mo re information, see

Drawing polylines and polygons

on page 8-163.

Rectangle Draw rectangles. Holding

square. Equivalent to the Rectangle command on the Place menu. For more information, see

S constrains t o a

Drawing rectangles and squares on page 8-160.

Ellipse Draw ellipses. Holding

to a circle. Equivalent to the Ellipse command on the Place menu. For more information, see

S constrains shape

Drawing circles and ellipses on page 8-161.

Chapter 2 The Capture work environment

Table 2 Tools on the schematic page editor tool palette (continued)

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.

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.

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

Table 3 Tools on the part editor tool palette

Tool Name Description

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

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 3 Tools on the part editor tool palette (continued)

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.

The tool palet te s

Chapter 2 The Capture work environment

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 pa le tte

1 From the schematic page editor’s View menu, choose

Tool Palette.

From the part editor’s View menu, choose Tool Palette.

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 status bar

The center field displays the number of items selected in the schematic page editor or part editor.

oteWhen a session log or a project

manager window is active, the center field of the status bar doesn’t display.

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 Si ze tab). The pointer location in the part editor is measured in grid units.

Chapter 2 The Capture work environment

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

1 From the schematic page editor’s View menu, choose

Status Bar.

From the part editor’s View menu, choose Status Bar.

Selecting and deselecting objects

Once you select an object, you can perf orm operati ons 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

1 Position the pointer on the object and click the left

mouse button. The object displays in the selection color.

To reset the selection color

1 From the Options menu, choose Preferences, then

select the Colors tab.

2 Click the left mouse button on the Selection color. 3 Click to select a color from the Selection Color

window, then click OK. Click OK again to dismiss the Preferences dialog box.

Note You can edit the properties of a

roup of objects using the property editor.

See The property editor on page 34.

To select multiple objects

1 For each object to select, position the pointer on the

object and hold button. Every object in the selection set displ ays in the selection color.

C while you click the left mouse

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.

To deselect objects

1 Click on the schematic page away from any objects.

Selected objects beco me deselected. Keep i n 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.

Chapter 2 The Capture work environment

To select all objects i n an area

1 From the tool palette, choose the selection tool. 2 Click on an area away from any objects or parts to

deselect any items that may be selected.

3 Move 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 yo ur selection rectangle

1 From the Options menu, choose Preferences. 2 On 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

1 From the Edit menu, choose Select All. All objects

appear in the selection color.

oteA selection set behaves as if it is 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 selectio n set,

ou could create a duplicate title block, or inadvertently move the title block off the schematic page.

To select an obje ct from a set o f object s stacke d atop o ne anoth er

1 Position the pointer over the stack of objects. 2 Press

F while you click the left mouse button. This

cycles through the objects in the stack.

To remove one object from a selection set

1 Place the pointer over the object, press C, and click

the left mouse button.

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 the m.

To group multiple selected objects

Selecting and deselecting objects

1 Select the objects you want to group. (See Selecting a nd

deselecting objects on page 2-26 for more information).

2 From the Edit menu, choose Group. You can move the

objects as a group.

3 When 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). Afte r block select ing the objects you want to group, desel e ct the included net aliases by holding the key and clicking on each object.

Chapter 2 The Capture work environment

Editing properties

In a Capture schematic design, each object has properti es 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.

Instance and occurrence properties

Since Capture allows for complex hierarchical design structures (as discussed in Chapter 6, 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.

Design structure),

Editing properties

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 plus (+) symbols in the property editor.

A change using any of the tools, like Annotate, also may update the instance property.

C key while clicking on one of the

Chapter 2 The Capture work environment

The Browse spreadsheet editor

You display the Browse spreadsheet editor from the project manager’s 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

Figure 13 Browse spreadsheet editor

• 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.

To create a new property in the Browse spreadsheet editor

1 In the first column of the Browse spreadsheet, select

the object or occurrence for which you want to create the new property.

2 From the Edit menu, choose Properties. Capture

displays the object in a new Browse spreadsheet window.

3 Click New. Capture displays the New Property dialog

box.

4 Enter a name and value for the new property, then

click OK. Capture adds the property to the object or occurrence and displays the new prope rty in the original Browse spreadsheet.

To copy a value from one prop erty to another proper ty in the Browse spreadsheet editor

1 In the first column of the Browse spreadsheet, select

the object or occurrence that has the property with the value you want to copy.

Editing properties

2 From the Edit menu, choose Properties. Capture

displays the object in a new Browse spreadsheet window.

3 Select the cell that contains the value you want to

copy.

4 Click Copy. 5 Select the cell that you want to contain the copied

value.

6 Click Paste. Capture pastes the value into the selected

cell.

Chapter 2 The Capture work environment

To remove a user-defined property in the Browse spread sheet editor

Note Some properties cannot be r emoved

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, th e 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.

1 In the first column of the Browse spreadsheet, select

the object or occurrence that has the property you want to remove.

2 Select the column heading for the property you want

to remove.

3 Click Remove. Capture removes that property from

the object.

To replace property values

1 Select 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.

2 From the Edit menu, choose Properties. The Browse

spreadsheet appears.

3 Double-click on a cell holding the value you wish to

replace, then enter the new value.

4 Click the copy button. 5 Select the cells that are to receive the replacement

value.

6 Click the Paste button. The replacement value appears

in the selected cells.

7 Click the OK button to close the Browse spreadsheet.

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

Editing properties

• 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.

Chapter 2 The Capture work environment

The property editor window

Note When you first st a rt the property

editor all instance proper ties are displayed. Occurrence properties are displayed only if they have their own values assigned to them (independent of the instance property values).

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.

Occurrence hierarchical path:reference

Instance name schematic name:page:reference

Property names

Item selection tabs

Filter drop-down list

Property value

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 th e 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

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 va lue 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 se t

the display options of the selected property and its value. You cannot display properties of an occurrence property using the Display Properties dialog box.

Editing properties

oteYou can pivot the property editor

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.

Delete Property Deletes the property, if editable, from

the selected object or objects. If you select all of a property’s 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.

Note Properties that are not editable

appear in italics.

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 Actel’s 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

Chapter 2 The Capture work environment

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, inclu ding 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 schema tic page that di splay s 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 alia ses at one time.

To pivot the property editor spreadsheet

1 Right-click the empty cell in the top-leftmost position

of the spreadsheet.

2 From the pop-up menu, choose Pivot.

To display or hide all occurrence properties

1 To display all occurrence properties, press and hold

C key while clicking on one of the plus (+)

the symbols in the left-most column.

2 To hide all occurrence properties, press and hold the

C key while clicking on one of the minus (-) symbols

in the left -most colu mn.

To move columns in the property editor

Editing properties

Note The Find command searches down

columns in the spreadsheet, regardless of the spreadsheet orientation.

1 Select the column you want to move by clicking on its

title cell.

2 Drag the column to the new location.

To sort columns in the property editor

1 Right-click on the column heading. A pop-up menu

appears.

2 Choose Sort Ascending or Sort Descending.

Note If the spreadsheet is pivoted, use

these steps to move rows.

Chapter 2 The Capture work environment

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 crea te 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 Captur e 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.

Undefined The selected property is not defined. It isn’t

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 Sp ecifies that any undefin ed

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 hi dden property col umns 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.

Editing properties

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.

Chapter 2 The Capture work environment

To create a new filter in the prope rt y edit or

1 Right-click any column heading in the spreadsheet. 2 Point to Filters in the pop-up menu and choose Add

Filter.

3 Type the new filter name in the Add Filter dialog box

and click OK. The new filter is saved in PREFPR OP.TXT wh en you close the property editor.

To edit a filter

1 Select a filter from the Filter by drop-down list. The

appearance of the properties on the spreadsheet may change when you change the filter.

2 Right-click any column heading and point to Filters in

the pop-up menu.

3 Use the Filters menu choices to change the property

definitions and appearance of the spreadsheet.

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.

Editing properties

To create a new property in th e property editor

1 In the schematic page editor, select the object(s) for

which you want to create the property.

2 From the Edit menu, choose Properties. Capture

displays the property editor.

3 Click the New Column or the New Row button.

Capture displays the Add New Column dialog box or the Add New Row dialog box.

4 Enter 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.

5 Enter values for the property as described in To edit a

property value in the property editor.

Chapter 2 The Capture work environment

Note Some property values (t hose that

have particular significance to th e design database) cannot be edited. Properties that are not editable appear in italics.

To edit a property val u e in th e property editor

1 In the property editor, select the cell that contains the

value you want to change.

2 Right-click and choose Edit from the pop-up menu.

The Edit Property Values dialog box appears.

3 Type in the new value and press

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.

R. Note that

To edit the a property value for all instances and occurrences currently displayed in the property editor

1 In the property editor, click the top-leftmost cell to

select the entire spreadsheet.

2 Right-click and choose Edit from the popup menu. 3 Select a property cell in the Edit Property Value dialog

box spreadsheet.

4 Type the new value for the property and click OK. The

new property value appears on the spreadsheet for all selected objects.

Note Some property values (t hose that

have particular significance to th e design database) cannot be deleted.

To delete a property in the property editor

1 Select the column of the property you want to delete. 2 Click 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.)

To display a property on the schematic page

Editing properties

1 In the property editor, select the instance property

cells you want to display, then click the Display button. Capture displays the Display Properties dialog box.

2 Complete 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 occurren ce.

Chapter 2 The Capture work environment

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 edi to r

The Package Properties spreadsheet editor is simi lar to the Browse spreadsheet editor with the following differences:

• The Package Properties spreadsheet editor doesn’t

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.

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 c hange 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 butt on 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 th e duplicate. The Validate button checks for duplicate pin numbers without requiring that you click OK.

Editing properties

Chapter 2 The Capture work environment

Note For description s of ot her ways to

manipulate objects, see Chapter 8, Adding and editing graphics and text.

Moving and resizing graphic objects

For some objects—such as wires, buses, lines, ellipses, rectangles, and so on—you can edit the object’s 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

1 Select the object to resize or move. 2 To 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.

To move the object, press the left mouse button anywhere on the object—except on a resize handle— and drag the object until it is where you want it. Release the mouse button.

3 To deselect the object, clic k i n an area whe re there a re

no parts or objects.

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

Undoing, redoing, and repeating an action

• Rotating objects

• Mirroring objects

To undo an action

1 From the Edit menu, choose Undo.

To reverse an undone acti on

1 From the Edit menu, choose Redo.

To repeat a command

1 Perform the command once. 2 From the Edit menu, choose Repeat.

ip You can use the R e peat command to

align objects or to quickly create repetitive structures such as buses.

Chapter 2 The Capture work environment

To repeat a copy operation

1 Select an object on a schematic page. 2 Press

3 From the Edit menu, choose Repeat. The pointer

C and drag the object to a new location. This

creates a copy of the object. Leave the object selected.

repeats the relative move in step 2 and an additional object is placed.

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 associ ates 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.

Using the Accessories menu

Chapter 2 The Capture work environment

Starting a project

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 library 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.

—it contains a copy of all the parts and symbols

Note Parts reside in a library the same

ay schematic pages reside in schematic folders. Symbols and title bl ocks also reside in libraries. A project can use any number of libraries, and a library can be in cluded in any number of projects. However, a project may have only one design (.DSN).

Chapter 3 Starting a project

w y

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 dial og 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 bl ocks, as well as schematic folders and the schematic pages cont ained 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

1 From the File menu, choose New, then choose Project.

The New Project dialog box appears.

2 Type a name for your new project in the Name text

box.

3 Use the Browse button to select a new directory.

Note The project types available to you

ill depend upon which Orcad programs

ou have installed. As a minimu m, you will have the option to create a PC Board o r Schematic project type.

4 Select 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 circuit—select 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.

• PC board—select 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 logic—select 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.

• Schematic—select 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

1 From the File menu, choose New, then choose Design. 2 The 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.

Creating new projec ts, designs, libraries, and VHDL files

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

ou want to replace the existing design.

To create a new schematic page

1 On the File tab of the project manager, select the

schematic folder that requires a new schematic page.

2 Click 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

1 From the File menu, choose New, then choose Library. 2 The 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.

For information on how to create p arts for inclusion in a library, see Chapter 12,

Creating and editing parts.

Chapter 3 Starting a project

To create a new VHDL file

There are two ways to create a new VHDL file in Capture:

1 From the File menu, choose New, then choose VHDL

File.

2 A VHDL file opens in Capture’s VHDL programmer’s

editor.

1 With the project manager active, choose New VHDL

File from the Design menu. The file opens in the VHDL programmer’s editor and a dialog box appears, asking if you want to add the file to the 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.

2 Choose the Yes button to add the file to the project that

is currently open. The Save As dialog box appears.

3 Select a directory for the file and supply a filename. By

default, the VHDL file’s name is VHDLn.VHD (where n is an integer indicating the number of .VHD files

created in the curre nt session).

4 Choose the Save button. Capture saves the file and

places it in the Design Resources folder of your project.

Opening existing projects,

designs, libraries, and VHDL files

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

1 From the File menu, point to Open, then choose

Project. The Open Project dialog box displays.

2 Select 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

1 From the File menu, point to Open, then choose

Design. The Open Design dialog box displays.

2 Select 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

1 In the project manager, select the File tab and

double- click the ico n of a schem atic folder ; this expands the folder and reveals the schematic pages it contains.

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, design, and

schematic page

2 Double-click on the icon of the schematic page you

want to open. The schematic page opens in a schematic page editor window.

Chapter 3 Starting a project

Figure 17 Open library

Figure 18 Open VHDL file

To open an existing library

1 From the File menu, point to Open, then choose

Library. The Open Library dialog box displays.

2 Select 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

1 From the File menu, point to Open, then choose VHDL

File. The Open VHDL File dialog box displays.

2 Select a VHDL file (.VHD) or type a name in the File

name text box, then choose the Open button. The VHDL file opens in Capture’s text editor.

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

1 In the project manager, select the folder to which you

want to add a file.

2 From the Edit menu, choose Project. The Add File to

Project Folder dialog box displays.

3 Select the file you want to add and choose the Open

button. The file is added to the project.

1 Drag the file from the Windows Explorer into the

folder in the project manager.

Working with files in a project

Note You can also add files to you r project

interactively. When you create a design using the New command on the File menu, it is placed in the project manager’s Design Resources folder.

To delete a file from a project

1 In the project manager, select the file you want to

delete.

2 Press the

project.

D key. The file is removed from the

Caution You will not be given a chance to

cancel this process after you pr ess the D key. If you delete a file by mistake,

ou will have to add it back to the project.

Chapter 3 Starting a project

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.

Note To avoid overwriting a design file

ith a misnamed project file, type in the filename without a file extension. Capture automatically saves the file with the correct file extension.

ip To protect your work in the event of a

system crash or power outage you ca n enable Auto Recovery, and set t h e in te rval 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 page’s design is saved, not the entire project. However, whe n 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.

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

1 With the design or library selected in the project

manager, from the File menu, choose Save. The Save As dialog box displays.

2 Enter a name for the design or library in the Fi le 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.

To save an existing project

1 With 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.

1 In the project manager, select the design file. 2 From the File menu, choose Save As. 3 Change the drive and directory as appropriate, then

select the file name and click Save.

4 Select the Design Resources folder. 5 From the File menu, choose Save As.

Closing a project

6 Change 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

1 From the project manager’s 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

1 From the project manager’s File menu, choose Exit.

Chapter 3 Starting a project

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.

Archiving a project

When the project manager window is active, you can archive a project. Archiving sa ves all file s 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

1 Make sure that the project you want to archive is

active.

2 From the project manager’s File menu, choose Archive

Project. The Archive Project dialog box appears.

Archiving a project

3 Select the types of additional files you want archived

with your project. If you don’t select any of the options (Library files, Output files, Re ferenced projects ), Capture automatically archives your project (*.OPJ) and design files (*.DSN).

4 Enter or browse to the directory in which you want to

archive your project.

5 Click 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.

Chapter 3 Starting a project

Setting up your project

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 Des ign

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 manager’s Options menu contains the Design Properties command, while the schematic page editor’s Options menu contains the Schematic Page Properties command.

Chapter 4 Setting up your project

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 i n the Capture initialization (.INI) file on your system. If you pass projects to others, they won’t 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 rema in, 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, it’s 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.

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 l ines 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.

Defining your pr eferences

• Select. Define whether you want to select objects

enclosed by a selection rectangle or obje cts inside and intersecting a selection recta ngle, 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.

Chapter 4 Setting up your project

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

1 From the Options menu, choose Preferences, then

choose the Colors/Print tab.

2 Select the check box by the color for the object to be

printed or plotted. Clear the check box f or the object to not be printed or plotted. Objects are always displayed on your screen, regardless of the setting of their check boxes.

To define an object’s color

1 From the Options menu, choose Preferences, then

choose the Colors/Print tab.

2 Click the left mouse button on the color of a n item. The

color palette window opens.

3 Select a new color. Click OK to dismiss the color

palette.

4 Click 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.

Defining your pr eferences

Note The color that you select for Title

Block is also t he co lor used for bord ers a nd

rid references.

Chapter 4 Setting up your project

Controlling the grid

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.

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

ip You can also show or hide th e grid

using the Grid command on the View menu in the schematic page editor or the part editor.

ip You can toggle the snap-to-grid using

the snap-to-grid tool bar button.

1 From the Options menu, choose Preferences, then

choose the Grid Display tab.

2 For 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.

3 Click OK.

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 window’s 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 independen tly.

Defining your pr eferences

Figure 21 Pan and Zoom tab of the Preferences dialog box

Chapter 4 Setting up your project

To configure zoom factor and auto scroll percent

1 From the Options menu, choose Preferences, then

choose the Pan and Zoom tab.

2 For 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.

ip You can also auto scroll without an

object attached to the pointer b y pressing the left mouse button as the pointer approaches the edge of the window.

• Auto Scroll Percent. Enter the percent of the

window’s horizontal or vertical dimen sion by which the display will scroll when the pointer approaches the edge of the window with an object attached.

3 Click OK.

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.

Defining your pr eferences

Figure 22 Select tab of the Preferences dialog box

To define selection options

1 From the Options menu, choose Preferences, then

choose the Select tab.

2 For 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 b y the selection border.

Chapter 4 Setting up your project

Note Capture may perform slower if you

set the Maximum number of objects to display at high resolution wh ile dragging t o a large number.

• 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.

3 Click OK.

Defining your pr eferences

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, whi ch is the method that Capture uses to communicate with other Orcad software, such as PSpice.

You can change the fill style, line style and

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 graphic s and text.

For information about intertool communication between Capture and Layout, see Chapter 19,

Capture with Orcad Layout.

For information about intertool communication between Capture and PSpice, see Chapter 20,

Capture with PSpice.

Using

Figure 23 Miscellaneous tab of the Preferences dialog box

To set miscellaneous options

1 From the Options menu, choose Preferences, then

choose the Miscellaneous tab.

2 For 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.

Chapter 4 Setting up your project

y y

• Line Style and Width. Select the line style and

width used for lines, polylines, rectangles, ell ipses, and arcs.

Note The Default color is the color defined

in the Graphics box in the Colors /Pr in t 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.

ip The Render TrueType fonts with

strokes option produces text that is prin ted or plotted quickly, but is not as aesthet ically pleasing as TrueType text. For this reason,

ou may want to enable the option when

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.

3 For the schematic page editor, set this option:

• Color. Select the color used for graphic object s

(rectangles, ellipses, and closed polylines).

4 Set the following options:

• Session L og. 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, styl e, 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.

• 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 hasn’t 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.

Defining your pr eferences

• 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 a s Orcad Layout and PSpice) in conjunction with Capture. Capture processes its tools faster w hen intertool communication is not selected.

5 Click OK.

Chapter 4 Setting up your project

Setting text editor options

Capture’s text editor options include automatic highlighting of VHDL keywords, comments, or quoted strings. You can also set the font, the tab sp acing, and enable or disable the highlighting feature.

Note The Highlight Keywords, Comments,

and Quoted Strings option must be enabled for Capture to use the syntax highlighting options.

Figure 24 Text Editor tab of the Preferences dialog box

To set text editor options

1 From the Options menu, choose Preferences, then

choose the Text Editor tab.

2 Set 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.

Orcad Capture User Guide

Specifications and Main Features

Frequently Asked Questions

User Manual

Contents

Before you begin

Welcome

How to use this guide

Getting started

Starting Capture

The Capture session frame

The Capture work environment

The project manager

The schematic page editor

The part editor

The programmer’s editor

The session log

The toolbar

The tool palettes

The status bar

Selecting and deselecting objects

Editing properties

Moving and resizing graphic objects

Undoing, redoing, and repeating an action

Using the Accessories menu

Starting a project

Creating new projects, designs, libraries, and VHDL files

Opening existing projects, designs, libraries, and VHDL files

Working with files in a project

Saving projects, designs, and libraries

Closing a project

Archiving a project

Setting up your project

Defining your preferences