Orcad PSPICE User Manual

OrCAD PSpice

User’s Guide

Trademarks

OrCAD, OrCAD Layout, OrCAD Express, OrCAD Capture, OrCAD PSpice, and OrCAD PSpice A/D are registered trademarks of OrCAD, Inc. OrCAD Capture CIS, and OrCAD Express CIS are trademarks of OrCAD, Inc.

Microsoft, Visual Basic, Windows, Windows NT, and other names of Microsoft products referenced herein are trademarks or registered trademarks of Microsoft Corporation.

All other brand and product names mentioned herein are used for identification purposes only, and are trademarks or registered trademarks of their respective holders.

Part Number 60-30-636 First edition 30 November 1998 Technical Support (503) 671-9400

Corporate offices (503) 671-9500 OrCAD Japan K.K. 81-45-621-1911 OrCAD UK Ltd. 44-1256-381-400 Fax (503) 671-9501 General email info@orcad.com Technical Support email techsupport@orcad.com World Wide Web http://www.orcad.com OrCAD Design Network (ODN) http://www.orcad.com/odn

9300 SW Nimbus Ave. Beaverton, OR 97008 USA

Before you begin xxiii

Welcome to OrCAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxiii

OrCAD PSpice overview . . . . . . . . . . . . . . . . . . . . . . . . . . xxiv

How to use this guide . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxv

Typographical conventions . . . . . . . . . . . . . . . . . . . . . . . xxv

Related documentation . . . . . . . . . . . . . . . . . . . . . . . . . . . xxvi

Online Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxvii

If you have the demo CD-ROM . . . . . . . . . . . . . . . . . . . . xxviii

OrCAD demo CD-ROM . . . . . . . . . . . . . . . . . . . . . . xxviii

What’s New . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxix

Part one Simulation primer

Things you need to know 1Chapter 1

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1

What is PSpice? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2

Analyses you can run with PSpice . . . . . . . . . . . . . . . . . . . . . . . 3

Basic analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

DC sweep & other DC calculations . . . . . . . . . . . . . . . . . . 3

AC sweep and noise . . . . . . . . . . . . . . . . . . . . . . . . . . 4

Transient and Fourier . . . . . . . . . . . . . . . . . . . . . . . . . . 5

Advanced multi-run analyses . . . . . . . . . . . . . . . . . . . . . . . 6

Parametric and temperature . . . . . . . . . . . . . . . . . . . . . . 6

Monte Carlo and sensitivity/worst-case . . . . . . . . . . . . . . . 7

Analyzing waveforms with PSpice . . . . . . . . . . . . . . . . . . . . . . 8

What is waveform analysis? . . . . . . . . . . . . . . . . . . . . . . . . 8

Using PSpice with other OrCAD programs . . . . . . . . . . . . . . . . . . 9

Using Capture to prepare for simulation . . . . . . . . . . . . . . . . 9

What is the Stimulus Editor? . . . . . . . . . . . . . . . . . . . . . . . 9

What is the Model Editor? . . . . . . . . . . . . . . . . . . . . . . . . . 10

Contents

Files needed for simulation . . . . . . . . . . . . . . . . . . . . . . . . . . 10

Files that Capture generates . . . . . . . . . . . . . . . . . . . . . . . 10

Netlist file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11

Circuit file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11

Other files that you can configure for simulation . . . . . . . . . . . 11

Model library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12

Stimulus file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

Include file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

Configuring model library, stimulus, and

include files . . . . . . . . . . . . . . . . . . . . . . . . . . 13

Files that PSpice generates . . . . . . . . . . . . . . . . . . . . . . . . . . 14

Waveform data file . . . . . . . . . . . . . . . . . . . . . . . . . . 14

PSpice output file . . . . . . . . . . . . . . . . . . . . . . . . . . . 14

Simulation examples 15Chapter 2

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15

Example circuit creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

Finding out more about setting up your design . . . . . . . . . . . . 21

Running PSpice . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22

Performing a bias point analysis . . . . . . . . . . . . . . . . . . . . . 22

Using the simulation output file . . . . . . . . . . . . . . . . . . . . . 24

Finding out more about bias point calculations . . . . . . . . . . . . 25

DC sweep analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26

Setting up and running a DC sweep analysis . . . . . . . . . . . . . . 26

Displaying DC analysis results . . . . . . . . . . . . . . . . . . . . . . 28

Finding out more about DC sweep analysis . . . . . . . . . . . . . . 31

Transient analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32

Finding out more about transient analysis . . . . . . . . . . . . . . . 36

AC sweep analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37

Setting up and running an AC sweep analysis . . . . . . . . . . . . . 37

AC sweep analysis results . . . . . . . . . . . . . . . . . . . . . . . . 39

Finding out more about AC sweep and noise analysis . . . . . . . . 41

Parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42

Setting up and running the parametric analysis . . . . . . . . . . . . 43

Analyzing waveform families . . . . . . . . . . . . . . . . . . . . . . 45

Finding out more about parametric analysis . . . . . . . . . . . . . . 48

Performance analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 49

Finding out more about performance analysis . . . . . . . . . . . . . 51

Part two Design entry

Preparing a design for simulation 55Chapter 3

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55

Checklist for simulation setup . . . . . . . . . . . . . . . . . . . . . . . . . 56

Typical simulation setup steps . . . . . . . . . . . . . . . . . . . . . . . 56

Advanced design entry and simulation setup steps . . . . . . . . . . . 57

When netlisting fails or the simulation

does not start . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58

Things to check in your design . . . . . . . . . . . . . . . . . . . . 58

Things to check in your system configuration . . . . . . . . . . . . 59

Using parts that you can simulate . . . . . . . . . . . . . . . . . . . . . . . 60

Vendor-supplied parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 61

Part naming conventions . . . . . . . . . . . . . . . . . . . . . . . . 61

Finding the part that you want . . . . . . . . . . . . . . . . . . . . 62

Passive parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64

Breakout parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65

Behavioral parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

Using global parameters and expressions for values . . . . . . . . . . . . 67

Global parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67

Declaring and using a global parameter . . . . . . . . . . . . . . . 67

Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69

Specifying expressions . . . . . . . . . . . . . . . . . . . . . . . . . 69

Defining power supplies . . . . . . . . . . . . . . . . . . . . . . . . . . . . 74

For the analog portion of your circuit . . . . . . . . . . . . . . . . . . . 74

Defining stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75

Analog stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75

Using VSTIM and ISTIM . . . . . . . . . . . . . . . . . . . . . . . . 76

If you want to specify multiple stimulus types . . . . . . . . . . . 77

Things to watch for . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 79

Unmodeled parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 79

Do this if the part in question is from the OrCAD libraries . . . . 79

Check for this if the part in question is custom-built . . . . . . . . 81

Unconfigured model, stimulus, or include files . . . . . . . . . . . . . 81

Check for this . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82

Unmodeled pins . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82

Check for this . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83

Missing ground . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83

Check for this . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83

Missing DC path to ground . . . . . . . . . . . . . . . . . . . . . . . . 84

Check for this . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 84

Contents

Creating and editing models 85Chapter 4

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85

What are models? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87

Models defined as model parameter sets . . . . . . . . . . . . . . 87

Models defined as subcircuit netlists . . . . . . . . . . . . . . . . 87

How are models organized? . . . . . . . . . . . . . . . . . . . . . . . . . 88

Model libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88

Model library configuration . . . . . . . . . . . . . . . . . . . . . . . 89

Global vs. design models and libraries . . . . . . . . . . . . . . . . . 89

Nested model libraries . . . . . . . . . . . . . . . . . . . . . . . . . . 90

OrCAD-provided models . . . . . . . . . . . . . . . . . . . . . . . . . 90

Tools to create and edit models . . . . . . . . . . . . . . . . . . . . . . . . 91

Ways to create and edit models . . . . . . . . . . . . . . . . . . . . . . . . 92

Using the Model Editor to

edit models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93

Ways to use the Model Editor . . . . . . . . . . . . . . . . . . . . . . 94

Model Editor-supported device types . . . . . . . . . . . . . . . . . . 95

Ways To Characterize Models . . . . . . . . . . . . . . . . . . . . . . 96

Creating models from data sheet information . . . . . . . . . . . 96

Analyzing the effect of model parameters

on device characteristics . . . . . . . . . . . . . . . . . . . 97

How to fit models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97

Running the Model Editor alone . . . . . . . . . . . . . . . . . . . . . 99

Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . . 99

Enabling and disabling automatic part creation . . . . . . . . . . 100

Saving global models (and parts) . . . . . . . . . . . . . . . . . . 100

Running the Model Editor from the schematic page editor . . . . . . 101

What is an instance model? . . . . . . . . . . . . . . . . . . . . . . 101

Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . . 102

Saving design models . . . . . . . . . . . . . . . . . . . . . . . . . 102

What happens if you don’t save the instance model . . . . . . . . 103

The Model Editor tutorial . . . . . . . . . . . . . . . . . . . . . . . . . 104

Creating the half-wave rectifier design . . . . . . . . . . . . . . . 104

Using the Model Editor to edit the D1 diode model . . . . . . . . 105

Entering data sheet information . . . . . . . . . . . . . . . . . . . 105

Extracting model parameters . . . . . . . . . . . . . . . . . . . . . 107

Adding curves for more than one temperature . . . . . . . . . . 108

Completing the model definition . . . . . . . . . . . . . . . . . . 109

Editing model text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110

Editing .MODEL definitions . . . . . . . . . . . . . . . . . . . . . 110

Editing .SUBCKT definitions . . . . . . . . . . . . . . . . . . . . . 111

Contents

Changing the model name . . . . . . . . . . . . . . . . . . . . . . 111

Starting the Model Editor

from the schematic page editor in Capture . . . . . . . . . . 111

What is an instance model? . . . . . . . . . . . . . . . . . . . . . 112

Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . 112

Saving design models . . . . . . . . . . . . . . . . . . . . . . . . 113

Example: editing a Q2N2222 instance model . . . . . . . . . . . . . . 114

Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . 114

Editing the Q2N2222-X model instance . . . . . . . . . . . . . . 114

Saving the edits and updating the schematic . . . . . . . . . . . 115

Using the Create Subcircuit command . . . . . . . . . . . . . . . . . . . 115

Changing the model reference to an existing model definition . . . . . . 117

Reusing instance models . . . . . . . . . . . . . . . . . . . . . . . . . . . 118

Reusing instance models in the same schematic . . . . . . . . . . . . 118

Making instance models available to all designs . . . . . . . . . . . 119

Configuring model libraries . . . . . . . . . . . . . . . . . . . . . . . . . 120

The Libraries and Include Files tabs . . . . . . . . . . . . . . . . . . . 120

How PSpice uses model libraries . . . . . . . . . . . . . . . . . . . . 121

Search order . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121

Handling duplicate model names . . . . . . . . . . . . . . . . . . 122

Adding model libraries to the configuration . . . . . . . . . . . . . . 122

Changing design and global scope . . . . . . . . . . . . . . . . . . . 123

Changing model library search order . . . . . . . . . . . . . . . . . . 124

Changing the library search path . . . . . . . . . . . . . . . . . . . . 125

Creating parts for models 127Chapter 5

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127

What’s different about parts used for simulation? . . . . . . . . . . . . . 129

Ways to create parts

for models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129

Preparing your models for part creation . . . . . . . . . . . . . . . . . . 130

Using the Model Editor to create parts . . . . . . . . . . . . . . . . . . . 131

Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . 131

Setting up automatic part creation . . . . . . . . . . . . . . . . . . . 132

Basing new parts on a custom set of parts . . . . . . . . . . . . . . . . . 133

Editing part graphics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135

How Capture places parts . . . . . . . . . . . . . . . . . . . . . . . . 135

Defining grid spacing . . . . . . . . . . . . . . . . . . . . . . . . . . . 136

Grid spacing for graphics . . . . . . . . . . . . . . . . . . . . . . 136

Grid spacing for pins . . . . . . . . . . . . . . . . . . . . . . . . . 136

Attaching models to parts . . . . . . . . . . . . . . . . . . . . . . . . . . 138

vii

Contents

MODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 138

Defining part properties needed for simulation . . . . . . . . . . . . . . 139

PSPICETEMPLATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140

PSPICETEMPLATE syntax . . . . . . . . . . . . . . . . . . . . . . 140

PSPICETEMPLATE examples . . . . . . . . . . . . . . . . . . . . 143

Analog behavioral modeling 147Chapter 6

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 147

Overview of analog behavioral modeling . . . . . . . . . . . . . . . . . . 148

The ABM.OLB part library file . . . . . . . . . . . . . . . . . . . . . . . . 149

Placing and specifying ABM parts . . . . . . . . . . . . . . . . . . . . . . 150

Net names and device names in ABM expressions . . . . . . . . . . 150

Forcing the use of a global definition . . . . . . . . . . . . . . . . . . 151

ABM part templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 152

Control system parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153

Basic components . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155

Limiters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156

Chebyshev filters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157

Integrator and differentiator . . . . . . . . . . . . . . . . . . . . . . . 160

Table look-up parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160

Laplace transform part . . . . . . . . . . . . . . . . . . . . . . . . . . 164

Math functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167

ABM expression parts . . . . . . . . . . . . . . . . . . . . . . . . . . 168

An instantaneous device example: modeling a triode . . . . . . . . . 171

PSpice-equivalent parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . 174

Implementation of PSpice -equivalent parts . . . . . . . . . . . . . . 175

Modeling mathematical or instantaneous relationships . . . . . . . . 176

EVALUE and GVALUE parts . . . . . . . . . . . . . . . . . . . . 176

EMULT, GMULT, ESUM, and GSUM . . . . . . . . . . . . . . . . 178

Lookup tables (ETABLE and GTABLE) . . . . . . . . . . . . . . . . . 179

Frequency-domain device models . . . . . . . . . . . . . . . . . . . . 181

Laplace transforms (LAPLACE) . . . . . . . . . . . . . . . . . . . . . 181

Frequency response tables (EFREQ and GFREQ) . . . . . . . . . . . 183

Cautions and recommendations for simulation and analysis . . . . . . . 186

Instantaneous device modeling . . . . . . . . . . . . . . . . . . . . . 186

Frequency-domain parts . . . . . . . . . . . . . . . . . . . . . . . . . 187

Laplace transforms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187

Non-causality and Laplace transforms . . . . . . . . . . . . . . . 188

Chebyshev filters . . . . . . . . . . . . . . . . . . . . . . . . . . . 190

Frequency tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . 190

Trading off computer resources for accuracy . . . . . . . . . . . . . . 191

viii

Basic controlled sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . 192

Creating custom ABM parts . . . . . . . . . . . . . . . . . . . . . . . 192

Part three Setting Up and Running Analyses

Setting up analyses and starting simulation 195Chapter 7

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 195

Analysis types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 196

Setting up analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 197

Execution order for standard analyses . . . . . . . . . . . . . . . . . 198

Output variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199

Modifiers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 200

Starting a simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 206

Starting a simulation from Capture . . . . . . . . . . . . . . . . . . . 206

Starting a simulation outside of Capture . . . . . . . . . . . . . . . . 207

Setting up batch simulations . . . . . . . . . . . . . . . . . . . . . . . 207

Multiple simulation setups within one circuit file . . . . . . . . . 207

Running simulations with multiple circuit files . . . . . . . . . . 208

The PSpice simulation window . . . . . . . . . . . . . . . . . . . . . 208

Contents

DC analyses 213Chapter 8

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 213

DC Sweep . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214

Minimum requirements to run a DC sweep analysis . . . . . . . . . 214

Overview of DC sweep . . . . . . . . . . . . . . . . . . . . . . . . . . 216

Setting up a DC stimulus . . . . . . . . . . . . . . . . . . . . . . . . . 218

Nested DC sweeps . . . . . . . . . . . . . . . . . . . . . . . . . . . . 219

Curve families for DC sweeps . . . . . . . . . . . . . . . . . . . . . . 221

Bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 223

Minimum requirements to run a bias point analysis . . . . . . . . . 223

Overview of bias point . . . . . . . . . . . . . . . . . . . . . . . . . . 223

Small-signal DC transfer . . . . . . . . . . . . . . . . . . . . . . . . . . . 225

Minimum requirements to run a small-signal DC transfer analysis . 225

Overview of small-signal DC transfer . . . . . . . . . . . . . . . . . . 226

DC sensitivity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 228

Minimum requirements to run a DC sensitivity analysis . . . . . . . 228

Overview of DC sensitivity . . . . . . . . . . . . . . . . . . . . . . . . 229

AC analyses 231Chapter 9

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 231

Contents

AC sweep analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 232

Setting up and running an AC sweep . . . . . . . . . . . . . . . . . . 232

What is AC sweep? . . . . . . . . . . . . . . . . . . . . . . . . . . . . 232

Setting up an AC stimulus . . . . . . . . . . . . . . . . . . . . . . . . 233

Setting up an AC analysis . . . . . . . . . . . . . . . . . . . . . . . . . 235

AC sweep setup in example.opj . . . . . . . . . . . . . . . . . . . . . 237

How PSpice treats nonlinear devices . . . . . . . . . . . . . . . . . . 239

What’s required to transform a device into a linear circuit . . . . 239

What PSpice does . . . . . . . . . . . . . . . . . . . . . . . . . . . 239

Example: nonlinear behavioral modeling block . . . . . . . . . . 239

Noise analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241

Setting up and running a noise analysis . . . . . . . . . . . . . . . . . 241

What is noise analysis? . . . . . . . . . . . . . . . . . . . . . . . . . . 242

How PSpice calculates total output

and input noise . . . . . . . . . . . . . . . . . . . . . . . . 242

Setting up a noise analysis . . . . . . . . . . . . . . . . . . . . . . . . 243

Analyzing Noise in the Probe window . . . . . . . . . . . . . . . . . 245

About noise units . . . . . . . . . . . . . . . . . . . . . . . . . . . 246

Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 246

Transient analysis 249Chapter 10

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 249

Overview of transient analysis . . . . . . . . . . . . . . . . . . . . . . . . 250

Minimum requirements to run a transient analysis . . . . . . . . . . 250

Minimum circuit design requirements . . . . . . . . . . . . . . . 250

Minimum program setup requirements . . . . . . . . . . . . . . 250

Defining a time-based stimulus . . . . . . . . . . . . . . . . . . . . . . . 252

Overview of stimulus generation . . . . . . . . . . . . . . . . . . . . 252

The Stimulus Editor utility . . . . . . . . . . . . . . . . . . . . . . . . . . 253

Stimulus files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253

Configuring stimulus files . . . . . . . . . . . . . . . . . . . . . . . . 254

Starting the Stimulus Editor . . . . . . . . . . . . . . . . . . . . . . . 254

Defining stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 256

Example: piecewise linear stimulus . . . . . . . . . . . . . . . . . 256

Example: sine wave sweep . . . . . . . . . . . . . . . . . . . . . . 257

Creating new stimulus symbols . . . . . . . . . . . . . . . . . . . . . 259

Editing a stimulus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 260

To edit an existing stimulus . . . . . . . . . . . . . . . . . . . . . 260

To edit a PWL stimulus . . . . . . . . . . . . . . . . . . . . . . . . 260

To select a time and value scale factor for PWL stimuli . . . . . . 260

Deleting and removing traces . . . . . . . . . . . . . . . . . . . . . . 261

Contents

Manual stimulus configuration . . . . . . . . . . . . . . . . . . . . . 261

To manually configure a stimulus . . . . . . . . . . . . . . . . . 261

Transient (time) response . . . . . . . . . . . . . . . . . . . . . . . . . . . 263

Internal time steps in transient analyses . . . . . . . . . . . . . . . . . . 265

Switching circuits in transient analyses . . . . . . . . . . . . . . . . . . . 266

Plotting hysteresis curves . . . . . . . . . . . . . . . . . . . . . . . . . . . 266

Fourier components . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 268

Parametric and temperature analysis 271Chapter 11

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271

Parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 272

Minimum requirements to run a parametric analysis . . . . . . . . . 272

Overview of parametric analysis . . . . . . . . . . . . . . . . . . . . 273

RLC filter example . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274

Entering the design . . . . . . . . . . . . . . . . . . . . . . . . . . 274

Running the simulation . . . . . . . . . . . . . . . . . . . . . . . 275

Using performance analysis to plot overshoot and rise time . . . 275

Example: frequency response vs. arbitrary parameter . . . . . . . . 278

Setting up the circuit . . . . . . . . . . . . . . . . . . . . . . . . . 278

Temperature analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 281

Minimum requirements to run a temperature analysis . . . . . . . . 281

Overview of temperature analysis . . . . . . . . . . . . . . . . . . . . 282

Monte Carlo and sensitivity/worst-case analyses 283Chapter 12

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 283

Statistical analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284

Overview of statistical analyses . . . . . . . . . . . . . . . . . . . . . 284

Output control for statistical analyses . . . . . . . . . . . . . . . . . . 285

Model parameter values reports . . . . . . . . . . . . . . . . . . . . . 285

Waveform reports . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 286

Collating functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 287

Temperature considerations in statistical analyses . . . . . . . . . . 288

Monte Carlo analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 289

Reading the summary report . . . . . . . . . . . . . . . . . . . . 291

Example: Monte Carlo analysis of a pressure sensor . . . . . . . . . 293

Drawing the schematic . . . . . . . . . . . . . . . . . . . . . . . . 293

Defining part values . . . . . . . . . . . . . . . . . . . . . . . . . 294

Setting up the parameters . . . . . . . . . . . . . . . . . . . . . . 295

Using resistors with models . . . . . . . . . . . . . . . . . . . . . 296

Saving the design . . . . . . . . . . . . . . . . . . . . . . . . . . . 297

Defining tolerances for the resistor models . . . . . . . . . . . . 297

Contents

Setting up the analyses . . . . . . . . . . . . . . . . . . . . . . . . 299

Running the analysis and viewing the results . . . . . . . . . . . 300

Monte Carlo Histograms . . . . . . . . . . . . . . . . . . . . . . . . . 301

Chebyshev filter example . . . . . . . . . . . . . . . . . . . . . . . 301

Creating models for Monte Carlo analysis . . . . . . . . . . . . . 302

Setting up the analysis . . . . . . . . . . . . . . . . . . . . . . . . 302

Creating histograms . . . . . . . . . . . . . . . . . . . . . . . . . . 303

Worst-case analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 306

Overview of worst-case analysis . . . . . . . . . . . . . . . . . . . . . 306

Inputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307

Procedure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307

Outputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 308

Caution: An important condition for

correct worst-case analysis . . . . . . . . . . . . . . . . . . 308

Worst-case analysis example . . . . . . . . . . . . . . . . . . . . . . . 309

Tips and other useful information . . . . . . . . . . . . . . . . . . . . 313

VARY BOTH, VARY DEV, and VARY LOT . . . . . . . . . . . . 313

Gaussian distributions . . . . . . . . . . . . . . . . . . . . . . . . 314

YMAX collating function . . . . . . . . . . . . . . . . . . . . . . . 314

RELTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 314

Sensitivity analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 314

Manual optimization . . . . . . . . . . . . . . . . . . . . . . . . . 314

Monte Carlo analysis . . . . . . . . . . . . . . . . . . . . . . . . . 315

Part four Viewing results

Analyzing waveforms 319Chapter 13

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319

Overview of waveform analysis . . . . . . . . . . . . . . . . . . . . . . . 320

Elements of a plot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 321

Elements of a Probe window . . . . . . . . . . . . . . . . . . . . . . . 322

Managing multiple Probe windows . . . . . . . . . . . . . . . . . . . 323

Printing multiple windows . . . . . . . . . . . . . . . . . . . . . . 323

Setting up waveform analysis . . . . . . . . . . . . . . . . . . . . . . . . . 324

Setting up colors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324

Editing display and print colors in the PSPICE.INI file . . . . . . 324

Configuring trace color schemes . . . . . . . . . . . . . . . . . . . 326

Viewing waveforms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 327

Setting up waveform display from Capture . . . . . . . . . . . . . . 327

Viewing waveforms while simulating . . . . . . . . . . . . . . . . . . 328

Configuring update intervals . . . . . . . . . . . . . . . . . . . . 329

xii

Contents

Interacting with waveform analysis during simulation . . . . . 329

Pausing a simulation and viewing waveforms . . . . . . . . . . 330

Using schematic page markers to add traces . . . . . . . . . . . . . . 331

Limiting waveform data file size . . . . . . . . . . . . . . . . . . . . 334

Limiting file size using markers . . . . . . . . . . . . . . . . . . . 334

Limiting file size by excluding intern al subcircuit data . . . . . . 336

Limiting file size by suppressing the first part

of simulation output . . . . . . . . . . . . . . . . . . . . . 336

Using simulation data from multiple files . . . . . . . . . . . . . . . 337

Appending waveform data files . . . . . . . . . . . . . . . . . . . 337

Adding traces from specific loaded waveform data files . . . . . 338

Saving simulation results in ASCII format . . . . . . . . . . . . . . . 339

Analog example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 341

Running the simulation . . . . . . . . . . . . . . . . . . . . . . . 341

Displaying voltages on nets . . . . . . . . . . . . . . . . . . . . . 343

User interface features for waveform analysis . . . . . . . . . . . . . . . 344

Zoom regions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 344

Scrolling traces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 346

Modifying trace expressions and labels . . . . . . . . . . . . . . . . . 346

Moving and copying trace names and expressions . . . . . . . . . . 347

Copying and moving labels . . . . . . . . . . . . . . . . . . . . . . . 348

Tabulating trace data values . . . . . . . . . . . . . . . . . . . . . . . 349

Using cursors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 350

Displaying cursors . . . . . . . . . . . . . . . . . . . . . . . . . . 350

Moving cursors . . . . . . . . . . . . . . . . . . . . . . . . . . . . 351

Example: using cursors . . . . . . . . . . . . . . . . . . . . . . . . 352

Tracking simulation messages . . . . . . . . . . . . . . . . . . . . . . . . 354

Message tracking from the message summary . . . . . . . . . . . . . 354

The Simulation Message Summary dialog box . . . . . . . . . . 354

Persistent hazards . . . . . . . . . . . . . . . . . . . . . . . . . . . 355

Message tracking from the waveform . . . . . . . . . . . . . . . . . . 356

Trace expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 356

Basic output variable form . . . . . . . . . . . . . . . . . . . . . . . . 357

Output variable form for device terminals . . . . . . . . . . . . . . . 358

Analog trace expressions . . . . . . . . . . . . . . . . . . . . . . . . . 364

Trace expression aliases . . . . . . . . . . . . . . . . . . . . . . . 364

Arithmetic functions . . . . . . . . . . . . . . . . . . . . . . . . . 364

Rules for numeric values suffixes . . . . . . . . . . . . . . . . . . 365

Other output opti ons 367Chapter 14

Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 367

xiii

Contents

Viewing analog results in the PSpice window . . . . . . . . . . . . . . . 368

Writing additional results to the PSpice output file . . . . . . . . . . . . 369

Generating plots of voltage and current values . . . . . . . . . . . . 369

Generating tables of voltage and current values . . . . . . . . . . . . 370

Setting initial state 373Appendix A

Appendix overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 373

Save and load bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . 374

Save bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 374

Load bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 375

Setpoints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 376

Setting initial conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 378

Convergence and “time step too small errors” 379Appendix B

Appendix overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 379

Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 380

Newton-Raphson requirements . . . . . . . . . . . . . . . . . . . . . 380

Is there a solution? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 381

Are the Equations Continuous? . . . . . . . . . . . . . . . . . . . . . 382

Are the derivatives correct? . . . . . . . . . . . . . . . . . . . . . 382

Is the initial approximation close enough? . . . . . . . . . . . . . . . 383

Bias point and DC sweep . . . . . . . . . . . . . . . . . . . . . . . . . . . 385

Semiconductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 385

Switches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 386

Behavioral modeling expressions . . . . . . . . . . . . . . . . . . . . 387

Transient analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 388

Skipping the bias point . . . . . . . . . . . . . . . . . . . . . . . . . . 389

The dynamic range of TIME . . . . . . . . . . . . . . . . . . . . . . . 389

Failure at the first time step . . . . . . . . . . . . . . . . . . . . . . . . 390

Parasitic capacitances . . . . . . . . . . . . . . . . . . . . . . . . . . . 391

Inductors and transformers . . . . . . . . . . . . . . . . . . . . . . . . 391

Bipolar transistors substrate junction . . . . . . . . . . . . . . . . . . 392

Diagnostics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 393

xiv

Index 395

Figures

Figure 1 User-configurable data files that PSpice reads . . . . . . . . . . . . . . . . 11

Figure 2 Diode clipper circuit. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

Figure 3 Connection points. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19

Figure 4 PSpice simulation output window. . . . . . . . . . . . . . . . . . . . . . . 22

Figure 5 Simulation output file. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24

Figure 6 DC sweep analysis settings. . . . . . . . . . . . . . . . . . . . . . . . . . . 27

Figure 7 Probe window. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28

Figure 8 Clipper circuit with voltage marker on net Out. . . . . . . . . . . . . . . . 29

Figure 9 Voltage at In, Mid, and Out. . . . . . . . . . . . . . . . . . . . . . . . . . . 29

Figure 11 Trace legend with cursors activated. . . . . . . . . . . . . . . . . . . . . . 30

Figure 12 Trace legend with V(Mid) symbol outlined. . . . . . . . . . . . . . . . . . 30

Figure 13 Voltage difference at V(In) = 4 volts. . . . . . . . . . . . . . . . . . . . . . 31

Figure 14 Diode clipper circuit with a voltage stimulus. . . . . . . . . . . . . . . . . 32

Figure 15 Stimulus Editor window. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 34

Figure 16 Transient analysis simulation settings. . . . . . . . . . . . . . . . . . . . . 34

Figure 17 Sinusoidal input and clipped output waveforms. . . . . . . . . . . . . . . 35

Figure 18 Clipper circuit with AC stimulus. . . . . . . . . . . . . . . . . . . . . . . . 37

Figure 19 AC sweep and noise analysis simulation settings. . . . . . . . . . . . . . . 38

Figure 20 dB magnitude curves for “gain” at Mid and Out. . . . . . . . . . . . . . . 40

Figure 21 Bode plot of clipper’s frequency response. . . . . . . . . . . . . . . . . . . 41

Figure 22 Clipper circuit with global parameter Rval. . . . . . . . . . . . . . . . . . 42

Figure 23 Parametric simulation settings. . . . . . . . . . . . . . . . . . . . . . . . . . 44

Ω

Figure 24 Small signal response as R1 is varied from 100

Figure 25 Small signal frequency response at 100 and 10 kΩ input resistance. . . . 47

Figure 26 Performance analysis plots of bandwidth and gain vs. Rval. . . . . . . . . 50

Figure 27 Relationship of the Model Editor to Capture and PSpice . . . . . . . . . . 93

Figure 28 Process and data flow for the Model Editor. . . . . . . . . . . . . . . . . . 96

Figure 29 Model Editor workspace with data for a bipolar transistor. . . . . . . . . 97

Figure 30 Design for a half-wave rectifier. . . . . . . . . . . . . . . . . . . . . . . . 104

Figure 31 Model characteristics and parameter values for DbreakX. . . . . . . . . 105

Figure 32 Assorted device characteristic curves for a diode. . . . . . . . . . . . . . 108

Figure 33 Forward Current device curve at two temperatures. . . . . . . . . . . . 109

to 10 k

Ω . . . . . . . . . . . 45

Figures

Figure 34 Rules for pin callout in subcircuit templates. . . . . . . . . . . . . . . . . 146

Figure 35 LOPASS filter example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157

Figure 36 HIPASS filter part example. . . . . . . . . . . . . . . . . . . . . . . . . . . 158

Figure 37 BANDPASS filter part example. . . . . . . . . . . . . . . . . . . . . . . . 159

Figure 38 BANDREJ filter part example. . . . . . . . . . . . . . . . . . . . . . . . . 159

Figure 39 FTABLE part example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162

Figure 40 LAPLACE part example one. . . . . . . . . . . . . . . . . . . . . . . . . . 165

Figure 41 Viewing gain and phase characteristics of a lossy integrator. . . . . . . . 165

Figure 42 LAPLACE part example two. . . . . . . . . . . . . . . . . . . . . . . . . . 165

Figure 43 ABM expression part example one. . . . . . . . . . . . . . . . . . . . . . 169

Figure 44 ABM expression part example two. . . . . . . . . . . . . . . . . . . . . . 169

Figure 45 ABM expression part example three. . . . . . . . . . . . . . . . . . . . . . 170

Figure 46 ABM expression part example four. . . . . . . . . . . . . . . . . . . . . . 170

Figure 47 Triode circuit. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 171

Figure 48 Triode subcircuit producing a family of I-V curves. . . . . . . . . . . . . 173

Figure 49 EVALUE part example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177

Figure 50 GVALUE part example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177

Figure 51 EMULT part example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 178

Figure 52 GMULT part example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 179

Figure 53 EFREQ part example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185

Figure 54 Voltage multiplier circuit (mixer). . . . . . . . . . . . . . . . . . . . . . . 186

Figure 55 PSpice simulation window . . . . . . . . . . . . . . . . . . . . . . . . . . 210

Figure 56 Example schematic EXAMPLE.OPJ. . . . . . . . . . . . . . . . . . . . . . 217

Figure 57 Curve family example schematic. . . . . . . . . . . . . . . . . . . . . . . 221

Figure 58 Device curve family. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 222

Figure 59 Operating point determination for each member of the curve family. . . 222

Figure 60 Circuit diagram for EXAMPLE.OPJ. . . . . . . . . . . . . . . . . . . . . . 237

Figure 61 AC analysis setup for EXAMPLE.OPJ. . . . . . . . . . . . . . . . . . . . . 238

Figure 62 Device and total noise traces for EXAMPLE.DSN. . . . . . . . . . . . . . 247

Figure 63 Transient analysis setup for EXAMPLE.OPJ. . . . . . . . . . . . . . . . . 263

Figure 64 Example schematic EXAMPLE.OPJ. . . . . . . . . . . . . . . . . . . . . . 264

Figure 65 ECL-compatible Schmitt trigger. . . . . . . . . . . . . . . . . . . . . . . . 266

Figure 66 Netlist for Schmitt trigger circuit. . . . . . . . . . . . . . . . . . . . . . . . 267

Figure 67 Hysteresis curve example: Schmitt trigger. . . . . . . . . . . . . . . . . . 268

Figure 68 Passive filter schematic. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274

Figure 69 Current of L1 when R1 is 1.5 ohms. . . . . . . . . . . . . . . . . . . . . . 276

Figure 70 Rise time and overshoot vs. damping resistance. . . . . . . . . . . . . . . 277

Figure 71 RLC filter example circuit. . . . . . . . . . . . . . . . . . . . . . . . . . . . 278

Figure 72 Plot of capacitance versus bias voltage. . . . . . . . . . . . . . . . . . . . 280

Figure 73 Example schematic EXAMPLE.OPJ. . . . . . . . . . . . . . . . . . . . . . 282

Figure 74 Example schematic EXAMPLE.DSN. . . . . . . . . . . . . . . . . . . . . 288

Figure 75 Monte Carlo analysis setup for EXAMPLE.DSN. . . . . . . . . . . . . . . 290

xvi

Figures

Figure 76 Summary of Monte Carlo runs for EXAMPLE.OPJ. . . . . . . . . . . . . 291

Figure 77 Parameter values for Monte Carlo pass three. . . . . . . . . . . . . . . . 292

Figure 78 Pressure sensor circuit. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 293

Figure 79 Model definition for RMonte1. . . . . . . . . . . . . . . . . . . . . . . . . 298

Figure 80 Pressure sensor circuit with RMonte1 and RTherm model definitions. . 299

Figure 81 Chebyshev filter. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 302

Figure 82 1 dB bandwidth histogram. . . . . . . . . . . . . . . . . . . . . . . . . . . 305

Figure 83 Center frequency histogram. . . . . . . . . . . . . . . . . . . . . . . . . . 306

Figure 84 Simple biased BJT amplifier. . . . . . . . . . . . . . . . . . . . . . . . . . 309

Figure 85 Amplifier netlist and circuit file. . . . . . . . . . . . . . . . . . . . . . . . 310

Figure 86 YatX Goal Function. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311

Figure 87 Correct worst-case results. . . . . . . . . . . . . . . . . . . . . . . . . . . 312

Figure 88 Incorrect worst-case results. . . . . . . . . . . . . . . . . . . . . . . . . . 312

Figure 89 Schematic using VARY BOTH. . . . . . . . . . . . . . . . . . . . . . . . . 313

Figure 90 Circuit file using VARY BOTH. . . . . . . . . . . . . . . . . . . . . . . . 313

Figure 91 Analog and digital areas of a plot. . . . . . . . . . . . . . . . . . . . . . . 321

Figure 92 Two Probe windows. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 322

Figure 93 Trace legend symbols. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 338

Figure 94 Section information message box. . . . . . . . . . . . . . . . . . . . . . . 339

Figure 95 Example schematic EXAMPLE.OPJ. . . . . . . . . . . . . . . . . . . . . . 341

Figure 96 Waveform display for EXAMPLE.DAT. . . . . . . . . . . . . . . . . . . 342

Figure 97 Cursors positioned on a trough and peak of V(1) . . . . . . . . . . . . . 352

Figure 98 Waveform display for a persistent hazard. . . . . . . . . . . . . . . . . . 355

Figure A-1 Setpoints. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 376

xvii

Figures

xviii

Tables

Table 1 DC analysis types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

Table 2 AC analysis types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4

Table 3 Time-based analysis types . . . . . . . . . . . . . . . . . . . . . . . . . . . 5

Table 4 Parametric and temperature analysis types . . . . . . . . . . . . . . . . . . 6

Table 5 Statistical analysis types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7

Table 2-1 25

Table 10 Association of cursors with mouse buttons. . . . . . . . . . . . . . . . . . 30

Table 2-1 31 Table 2-1 36 Table 2-2 41 Table 2-3 48 Table 2-4 51 Table 5 58 Table 6 59

Table 7 Passive parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64

Table 8 Breakout parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65

Table 9 Operators in expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70

Table 10 Function s in arithmetic expressions . . . . . . . . . . . . . . . . . . . . . . 71

Table 11 System variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73

Table 12 74 Table 13 75 Table 14 77 Table 15 78 Table 16 80

Table 17 Models supported in the Model Editor . . . . . . . . . . . . . . . . . . . 95

Table 1 Sample diode data sheet values . . . . . . . . . . . . . . . . . . . . . . . 106

Table 2 Part names for custom part generation. . . . . . . . . . . . . . . . . . . . 133

Table 3 139 Table 4 141 Table 5 142 Table 6 145

Table 7 Control system parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153

Tables

Table 1 ABM math function parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 167

Table 2 ABM expression parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168

Table 1 PSpice -equivalent parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 174

Table 1 Basic controlled sources in ANALOG.OLB . . . . . . . . . . . . . . . . . 192

Table 2 Classes of PSpice analyses . . . . . . . . . . . . . . . . . . . . . . . . . . 196

Table 3 Execution order for standard analyses . . . . . . . . . . . . . . . . . . . . 198

Table 4 PSpice output variable formats . . . . . . . . . . . . . . . . . . . . . . . 201

Table 5 Element definitions for 2-terminal devices . . . . . . . . . . . . . . . . . 202

Table 6 Element definitions for 3- or 4-terminal devices . . . . . . . . . . . . . . 203

Table 7 Element definitions for transmission line devices . . . . . . . . . . . . . 204

Table 8 Element definitions for AC analysis specific elements . . . . . . . . . . 205

Table 9 DC sweep circuit design requirements . . . . . . . . . . . . . . . . . . . 214

Table 10 218 Table 11 218 Table 12 219

Table 1 Curve family example setup . . . . . . . . . . . . . . . . . . . . . . . . . 221

Table 2 233 Table 3 233 Table 4 234 Table 5 234 Table 6 236 Table 7 242 Table 8 244 Table 9 246

Table 10 Stimulus symbols for time-based input signals . . . . . . . . . . . . . . 252

Table 1 Parametric analysis circuit design requir ements . . . . . . . . . . . . . . 272

Table 1 Collating functions used in statistical analyses . . . . . . . . . . . . . . . 287

Table 1 294 Table 2 295 Table 3 300

Table 1 Default waveform viewing colors. . . . . . . . . . . . . . . . . . . . . . . 325

Table 2 326 Table 3 328 Table 4 330 Table 5 332 Table 6 333 Table 1 346

Table 2 Mouse actions for cursor control . . . . . . . . . . . . . . . . . . . . . . . 351

Table 3 Key combinations for cursor control . . . . . . . . . . . . . . . . . . . . 351

Table 4 357 Table 5 358

Table 6 Output variable formats . . . . . . . . . . . . . . . . . . . . . . . . . . . 358

Tables

Table 7 Examples of output variable formats . . . . . . . . . . . . . . . . . . . . 360

Table 8 Output variable AC suffixes . . . . . . . . . . . . . . . . . . . . . . . . . 361

Table 9 Device names for two-terminal device types . . . . . . . . . . . . . . . 361

Table 10 Terminal IDs by three & four-terminal device type . . . . . . . . . . . . 362

Table 11 Noise types by device type . . . . . . . . . . . . . . . . . . . . . . . . . . 363

Table 12 Analog arithmetic functions for trace expressions . . . . . . . . . . . . 364

Table 13 Output units for trace expressions . . . . . . . . . . . . . . . . . . . . . 366

Table 14 369 Table 15 370

xxi

Tables

xxii

Before you begin

Welcome to OrCAD

OrCAD® offers a total solution for your core design tasks: schematic- and VHDL-based design entry; FPGA and CPLD design synthesis; digital, analog, and mixed-signal simulation; and printed circuit board layout. What's more, OrCAD's products are a suite of applications built around an engineer's design flow--not just a collection of independently developed point tools. PSpice is just one element in OrCAD's total solution design flow.

With OrCAD’s products, you’ll spend less time dealing with the details of tool integration, devising workarounds, and manually entering d ata to keep file s in sync. Our products will help you build better products faster, and at lower cost.

Before you begin

OrCAD PSpice overview

OrCAD PSpice simulates analog-only circuits. After you prepare a design for simulation, OrCAD Capture generates a circuit file set. The circuit file set, containing the circuit netlist and analysis commands, is read by PSpice for simulation. PSpice formulates these into meaningful graphical plots, which you can mark for display directly from your schematic page using markers.

xxiv

How to use this guide

This guide is designed so you can quickly find the information you need to use PSpice.

This guide assumes that you are familiar with Microsoft Windows (NT or 95), including how to use icons, menus, and dialog boxes. It also assumes you have a basic understanding about how Windows manages applications and files to perform routine tasks, such as starting applications, and openin g and saving your work. If you are new to Windows, please review your Microsoft Windows User’s Guide.

Typographical conventions

Before using PSpice, it is important to understand the terms and typographical conventions used in this documentation.

How to use this guide

This guide generally follows the conventions used in the Microsoft Win dows User’s Guide. Procedures for performing an operation are generally numbered with the following typographical conventions..

Notation Examples Description

C+r

monospace font

Press C+

Type

VAC...

A specific key or key stroke on the keyboard.

. Commands/te xt entered

from the keyborad.

xxv

Before you begin

What’s New

New PSpice interface with integrated waveform analysis functionality Release 9 of PSpice incl udes all

of Probe’s features and adds to them. Included in one screen are tabbed windows for viewing plots, text windows for viewing output files or other text files, and a simulation status and message window. Also included is a new, self-documenting analysis setup dia log for creating simulation profiles (see below). PSpice now provides an editable simulation queue which shows you how many files are currently in line to be simulated. You can edit or re-order the list as needed. And the plotting features have been improved by providing user-controlled grid setti ngs, grid and trace properties (style and color) and metafile format copy and paste functions.

Simulation profiles PSpice Release 9 introduces the

concept of simulation profiles. Each simulation profile refers to one schematic in a design and includes one analysis type (AC, DC, or Transient) with any options (sensitivity, temperature, parametric, Monte Carlo, etc.). You can define as many profiles as you need for your design and you can set up multiple analyses of the same type. Simulation profiles help you keep your analysis results separate, so you can delete one without losing the rest.

To find out more, see Analyzing

waveforms on page -319.

New OrCAD Capture front-end Release 9 integrates

OrCAD Capture as the front-end schematic entry tool for PSpice. Capture provides a professional design entry environment with many advanced capabilities that now work hand-in-hand with PSpice. These include a project manager, a new property editor spreadsheet, right mouse button support, and many other time-saving features.

xxix

Before you begin

To find out more, see Creating and

editing models on page -85.

To find out more, refer to MOSFET devices in the Analog Devices chapter of the online OrCAD PSpice A/D

eference Manual.

New Model Editor interface The Model Editor

(formerly known as Parts) has been improved and modernized for Release 9. It now provides a unified application for editing models either in text form or by modifying their specifications. The Model Editor now also supports Darlington modeling.

EKV version 2.6 MOSFET model The EKV model is a

scalable and compact model built on fundamental physical properties of the device. Use this model to design low-voltage, low-current analog, and mixed analogdigital circuits that use sub-micron technologies.

Version 2.6 models the fo llowing:

• geometrical and process related aspects of the device

(oxide thickness, junction depth, effective channel length and width, and so on)

• effects of doping profile and substrate effects

• weak, moderate, and strong inversion behavior

• mobility effects due to vertical and lateral fields and

carrier velocity saturation

• short-channel effects such as channel-length

modulation, source and drain charge sharing, and the reverse short channel effect

• thermal and flicker noise modeling

• short-distance geometry and bias-dependent device

matching for Monte Carlo analysis

Enhanced model libraries The model libraries

supplied with PSpice Release 9 have been enhanced to include the latest models from various vendors, as well as models for popular optocouplers, Darlingtons, and DAC and ADC devices.

xxx

Part one

Simulation primer

Part one provides basic information about circuit simulation including examples of common analyses.

• Chapte r 1, Things you need to know, provides an

overview of the circuit simulation process including what PSpice does, descriptions of analysis types, an d descriptions of important files.

• Chapte r 2, Simulation examples, presents examples of

common analyses to introduce the methods and tools you’ll need to enter, simulate, and analyze your design.

Things you need to know

Chapter overview

This chapter introduces the purpose and function of the OrCAD

• What is PSpice? on page 1-2 describes PSpice

• Analyses you can ru n wit h PS pic e on page 1-3 introduces

•

PSpice circuit simulator.

capabilities.

the different kinds of basic and advanced analyses that PSpice supports.

Using PSpice with other OrCAD programs on page 1-9

presents the high-level simulation design flow.

Files needed for simulation on page 1-10 describes the

files used to pass information between OrCAD programs. This section also introduces the things you can do to customize where and how PSpice finds simulation information.

Files that PSpice generates on page 1-14 describes the

files that contain simulation results.

Chapter 1 Things you need to know

What is PSpice?

OrCAD PSpice is a simulation program that models the behavior of a circuit containin g analog devices. Used with OrCAD Capture for design entry, you can think of PSpice as a software-based breadboard of your circuit that you can use to test and refine your design before ever touching a piece of hardware.

Run basic and advanced analyses PSpice can

perform:

• DC, AC, and transient analyses, so you can test the

response of your circuit to different inputs.

• Parametric, Monte Carlo, and sensitivity/worst-case

analyses, so you can see how your circuit’s behavior varies with changing component values.

The range of models built into PSpice include not only those for resistors, inductors, capacitors, and bipolar transistors, but also these:

• transmission line models, including

delay, reflection, loss, dispersion, and crosstalk

• nonlinear magnetic core models,

including saturation and hysteresis

•

six MOSFET models, including BSIM3 version 3.1 and EKV version 2.6

•

five GaAsFET models, includ ing Parker-Skellern and TriQuint’s TOM2 model

•

IGBTs

Use parts from OrCAD’s extensive set of libraries

The model libraries feature over 11,300 analog models of devices manufactured in North America, Japan, and Europe.

Vary device characteristics without creating new parts PSpice has numerous built-in models with

parameters that you can tweak for a given device. These include independent temperature effects.

Model behavior PSpice supports analog behavioral

modeling, so you can describe functional blocks of circuitry using mathematical expressions and functions.

Analyses you can run wi th PSpice

Analyses you can run with PSpice

Basic analyses

DC sweep & other DC calculations

These DC analyses evaluate circuit performance in response to a direct current source. Table 1 what PSpice calculates for each DC analysis type.

Table 1 DC analysis types

For this DC analysis... PSpice computes this. ..

DC sweep Steady-state voltages and currents

when sweeping a source, a model parameter, or temperature over a range of values.

Bias point detail Bias point data in addition to what is

automatically computed in any simulation.

summarizes

See Chapter 2,

examples

showing how to run each type of analysis. See Part t hree

unning Analyses, for a more detailed discussion of each type of analysis and how to set it up.

Simulation

, for introductory examples

, Setting Up and

DC sensitivity Sensitivity of a net or part voltage a s a

function of bias point.

Small-signal DC transfer

Small-signal DC gain, input resistance, and output resistance as a function of bias point.

Chapter 1 Things you need to know

AC sweep and noise

These AC analyses evaluate circuit performance in response to a small-signal alternating current source.

Table 2

analysis type.

summarizes what PSpice calculates for each AC

Table 2

Note

AC analysis types

For this AC analysis... PSpice computes this. ..

AC sweep Small-signal response of the circuit

(linearized around the bias point) when sweeping one or more sources over a range of frequencies. Outputs include voltages and currents with magnitude and phase; you can use this information to obtain Bode plots.

Noise For each frequency specified in the AC

analysis:

Propagated no ise contributi ons at an

•

output net from every noise generator in the circuit.

RMS sum of the noise contributions

•

at the output. Equivalent input noise.

•

To run a noise analysis, you must also run an AC sweep analysis.

Transient and Fourier

These time-based analyses evaluate circui t performance in response to time-varying sources. Table 3 what PSpice calculates for each time-based analysis type.

summarizes

Analyses you can run wi th PSpice

Table 3

Note

Time-bas ed analysis types

For this time-bas e d analysis... PSpice computes this...

Transient Voltages and currents tracked over

time.

Fourier DC and Fourier components of the

transient analysis results.

To run a Fourier analysis, you must also run a transient analysis.

Chapter 1 Things you need to know

Advanced multi-run analyses

The multi-run analyses—parametric, temperature, Monte Carlo, and sensitivity/worst-case—result in a series of DC sweep, AC sweep, or transient analyses depending on which basic analyses you enabled.

Parametric and temperature

For parametric and temperature analyses, PSpice steps a circuit value in a sequence that you specify and runs a simulation for each value.

Table 4

kind of analysis.

Table 4 Parametric and temperature analysis types

shows the circuit values that you can ste p for each

For this analysis... You can step one of these...

Parametric global parameter

model parameter component value DC source operational temperature

Temperature operational temperature

Monte Carlo and sensitivity/worst-case

Monte Carlo and sensitivity/worst-case analyses are statistical. PSpice changes device model parameter values with respect to device and lot tolerances that you specify, and runs a simulation for each valu e.

Analyses you can run wi th PSpice

Table 5

summarizes how PSpice runs each statistical

analysis type.

Table 5 Statistical analysis types

For this statistical analysis... PSpice does this...

Monte Carlo For each simulation,

device model parameters for which you have defined a tolerance.

Sensitivity/ worst-case

Computes the probable worst-case response of the circuit in two steps:

Computes component sensitiv ity to

changes in the device model parameters. This means PSpice

nonrandomly

parameters for which you have defined a tolerance, one at a time for each device and runs a simulation with each change.

Sets

devices to their worst-case values (assumed to be at one of the tolerance limits) and runs a final simulation.

model parameters for

all

r a ndomly

varies device model

varies all

all

Chapter 1 Things you need to know

Taken together, simulation and waveform analysis is an iterative process. After analyzing simulation results, you can refine your design and simulation settings and then perform a new simulation and waveform analysis.

Analyzing waveforms with PSpice

What is waveform analysis?

After completing the simulation, PSpice plots the waveform results so you can visualize the circuit’s behavior and determine the validity of your design.

Perform post-simulation analysis of the results This means you can plot addition al information

derived from the waveforms. What you can pl ot depends on the types of analyses you run. Bode plots, phase margin, derivatives for small-signal characteristics, waveform families, and histograms are only a few of the possibilities. You can also plot other waveform characteristics such as rise time versus temperature, or percent overshoot versus component value.

Using PSpice with other OrCAD programs

Using Capture to prepare for simulation

Capture is a design entry program you need to prepare your circuit for simulation. This means:

• placing and connecting part symbols,

• defining component values and other attributes,

• defining input waveforms,

• enabling one or more analyses, and

• marking the points in the circuit where you want to

see results.

Capture is also the control point for running other programs used in the simulation design flow.

Using PSpice with other OrCAD programs

What is the Stimulus Editor?

The Stimulus Editor is a graphical in put waveform edi tor that lets you define the shape of time-based signals used to test your circuit’s response during simulation. Using the Stimulus Editor, you can define:

•

analog stimuli with sine wave, pulse, piecewise l inear, exponential pulse, single-frequency FM shapes

The Stimulus Editor lets you draw analog piecewise linear stimuli by clicking at the points along the timeline that correspond to the input values that you want at transitions.

Chapter 1 Things you need to know

What is the Model Editor?

The Model Editor is a model extractor that generates model definitions for PSpice to use during simulation. All the Model Editor needs is information about the device found in standard data sheets. As you enter the data sheet information, the Model Editor displays device characteristic curves so you can verify the model-based behavior of the device. When you are finished, the Mode l Editor automatically creates a part for the model so you can use the modeled part in your design immediately.

Files needed for simulation

To simulate your design, PSpice needs to know about:

• the parts in your circuit and how they are connected,

• what analyses to run,

• the simulation models that correspond to the parts in

your circuit, and

• the stimulus definitions to test with.

This information is provided in various data files. Some of these are generated by Capture, others come from libraries (which can also be generated by other programs like the Stimulus Editor and the Model Editor), and still others are user-defined.

Files that Capture generates

When you begin the simulation process, Capture first generates files describing the parts and connections in your circuit. These files are the netlist file and the circuit file that PSpice reads before doing anything else.

Netlist file

Files needed for simula t ion

The netlist file contains a li st of device na mes, values, and how they are connected with other devices. The name that Capture generates for this file is DESIGN_NAME.NET.

Circuit file

The circuit file contains commands describing how to run the simulation. This file also refers to other files that contain netlist, model, stimulus, and any other user-defined information that apply to the simulation. The name that Capture generates for this file is DESIGN_NAME.CIR.

Other files that you can configure for simulation

OrCAD Stimulus Editor

global model

libraries

OrCAD Model Editor

MODEL

+BF=

model definitions

input waveforms

Refer to the online OrCAD PSpice

eference Manual for the syntax of the statements in the netlist file and the circuit file.

stimulus file

simulation primitives

local model

libraries

OrCAD PSpice

custom include file

Figure 1 User-configurable data files that PSpice reads

Before starting simulation, PSpice needs to read other files that contain simulation informa tion for your circuit. These are model files, and if required, stimulus files and include files.

The circuit file (.CIR) that Capture generates contains references to the other user-configurable files t hat PSpice needs to read.

Chapter 1 Things you need to know

You can create these files using OrCAD programs like the Stimulus Editor and the Model Editor. These programs automate file generation and provide graphical ways to verify the data. You can also use the Model Text view in the Model Editor (or another text editor like Notepad) to enter the data manually.

Model library

A model library is a file that contains the electrical definition of one or more parts. PSpice uses this information to determine how a part will respond to different electrical inputs.

These definitions take the form of either a:

• model parameter set, which defines the behavior of a

part by fine-tuning the underlying model built into PSpice, or

A subcircuit, sometimes called a macr omodel, is analogous to a procedure call in a software programming language.

See What is the Model Editor?

on page 1-10 for a description.

• subcircuit netlist, which describes the structure and

function of the part by interconnecting other parts and primitives.

The most commonly used models are available in the OrCAD model libraries shipped with your programs. The model library names have a .LIB extension.

If needed, however, you can create your own models and libraries, either:

• manually using the Model Text view in the Model

Editor (or another text editor like Notepad), or

•

automatically using the Model Editor.

Stimulus file

Files needed for simula t ion

A stimulus file contains time-based definitions for analog input waveforms. You can create a stimulus file either:

• manually using the Model Text View of the Model

Editor (or a standard text editor) to create the definition (a typical file extension is .STM), or

• automatically using the Stimulus Editor (which

generates a .STL file extension).

Include file

An include file is a user-defined file that contains:

• PSpice commands, or

• supplemental text comments that you want to appear

in the PSpice output file (see page 1-14

You can create an include file using any text editor, such as Notepad. Typically, include file names have a .INC extension.

Configuring model library, stimulus, and include files

PSpice searches model libraries, stimulus files, and include files for any information it needs to complete the definition of a part or to run a simulation.

Note

Not all stimulus definitions require a stimulus file. In some cases, like DC and AC sources, you must use a schematic symbol and set its attribut es.

ee What is the Stimulus Editor?

on page 1-9 for a description.

Example: An include file that contains definitions, using the PSpice .FUNC command, for functions that you want to use in numeric expressions elsewhere in your design.

Files that PSpice generates

After reading the circuit file, netlist file, model libraries, and any other required inputs, PSpice starts the simulation. As simulation progresses, PSpice saves res ults to two files—the data file and the PSpice output file.

For a description of how to display simulation results, see Part four Viewing results.

For a description of the wav eform analyzer program, see What is waveform

analysis? on page 1-8.

There are two ways to add waveforms to the display:

• From within PSpice, by specifying trace

expressions.

• From within Capture, by cross-probing.

Waveform data file

The data file contains simulation results that that can be displayed graphically. PSpice reads this file automatic ally and displays waveforms reflecting circuit response at nets, pins, and parts that you marked in your schematic (cross-probing). You can set up your design so PSpice displays the results as the simulation progresses or after the simulation completes.

After PSpice has read the data f ile an d displays the initial set of results, you can add more waveforms and to perform post-simulation analysis of the data.

PSpice output file

The PSpice output file is an ASCII text file that contains:

• the netlist representation of the circuit,

• the PSpice command syntax for simulati on commands

and options (like the enabled analyses),

•

simulation results, and

• warning and error messages for problems

encountered during read-in or simulation.

Example: Each instance of a VPRINT1 symbol placed in your schematic causes PSpice to generate a ta ble of voltage values for the connecting ne t, and to write the table to the PSpice output file.

Its content is determined by:

•

the types of analyses you run,

•

the options you select for running PSpice, and

•

the simulation control symbols (like VPRINT1 and VPLOT1) that you place and connect to nets in your design.

Simulation examples

Chapter overview

The examples in this chapter provide an introduction to the methods and tools for creating circuit designs, running simulations, and analyzing simulation results. All analyses are performed on the same example circuit to clearly illustrate analysis setup, simulation, and result-analysis procedures for each analysis type.

This chapter includes the following sections:

•

Example circuit creation on page 2-16

•

Performing a bias point analysis on page 2-22

•

DC sweep an alysis on page 2-26

•

Transient analysis on page 2-32

•

AC sweep an alysis on page 2-37

•

Parametric analysis on page 2-42

•

Performance analysis on page 2-49

Chapter 2 Simulation examples

Example circuit creation

This section describes how to use OrCAD Capture to create the simple diode clipper circuit shown in Figure 2.

Figure 2 Diode clipper circuit.

To create a new PSpice project

1 From the Windows Start menu, choose the OrCAD

Release 9 program folder and then the Capture shortcut to start Capture.

2 In the Project Manager, from the File menu, point to

New and choose Project.

3 Select Analog Circuit Wizard. 4 In the Name text box, enter the name of the project

(CLIPPER).

5 Click OK, then click Finish.

No special libraries need to be configured at thi s time. A new page will be displayed in Capture and the new project will be configured in the Project Manager.

To place the voltage sources

1 In Capture, switch to the schematic page editor.

Example circuit creation

2 From the Place menu, choose Part to display the Place

Part dialog box.

3 Add the library for the parts you need to place:

a Click the Add Library button. b Select SOURCE.OLB (from the PSpice library) and

click Open.

4 In the Part text box, type

VDC.

5 Click OK. 6 Move the pointer to the correct position on the

schematic page (see Figure 2) and click to place the first part.

7 Move the cursor and click again to place the second

part.

8 Right-click and choose End Mode to stop placing

parts.

To place the diodes

1 From the Place menu, choose Part to display the Place

Part dialog box.

Note

There are two sets of library files supplied with Capture and PSpice. The standard schematic part libraries are found in the directory Capture\Library. The part libraries that are desi gned for simulation with PSpice are found in the sub-directory Capture\Library\PSpice. In order to have access to specific parts, you mus t fir st configure the library in Capture using the Add Library function.

2 Add the library for the parts you need to place:

a Click the Add Library button. b Select DIODE.OLB (from the PSpice library) and

click Open.

3 In the Part text box, type

D1N39 to display a list of

diodes.

4 Select D1N3940 and click OK. 5 Press r to rotate the diode to the correct orientation. 6 Click to place the first diode (D1), then click to place

the second diode (D2).

7 Right-click and choose End Mode to stop placing

parts.

When placing parts:

•

Leave space to connect the parts with wires.

•

You will change part names an d values that do not match those shown in Figure 2 later in this section.

Chapter 2 Simulation examples

To move the text associated with the diodes (or any other object)

1 Click the text to select it, then drag the text to a new

location.

To place the other parts

pre

1 From the Place menu, choose Part to display the Place

Part dialog box.

2 Add the library for the parts you need to place:

a Click the Add Library button. b Select ANALOG.OLB (from the PSpice library)

and click Open.

3 Follow similar steps as described for the diodes to

place the parts listed below, ac cording to Figure 2. The part names you need to type in the Part name text box of the Place Part dialog box are shown in parentheses:

• resistors (R)

• capacitor (C)

4 To place the off-page connector parts

(OFFPAGELEFT-R), click the Place Off-Page Connector button on the tool palette.

5 Add the library for the parts you need to place:

a Click the Add Library button. b Select CAPSYM.OLB (from the Capture library)

and click Open.

6 Place the off-page connector parts according to

Figure 2.

7 To place the ground parts (0), click the GND button on

the tool palette.

8 Add the library for the parts you need to place:

a Click the Add Library button. b Select SOURCE.OLB (from the PSpice library) and

click Open.

9 Place the ground parts according to Figure 2.

To connect the parts

Example circuit creation

1 From the Place menu, choose Wire to begin wiring

parts. The pointer changes to a crosshair.

2 Click the connection point (the very end) of the pin on

the off-page connector at the input of the circuit.

3 Click the nearest connection point of the input resistor

R1.

4 Connect the other end of R1 to the output capacitor. 5 Connect the diodes to each other and to the wire

between them:

a Click the connection point of the cathode for the

lower diode.

b Move the cursor straight up and click the wire

between the diodes. The wire ends, and the junction of the wire segments becomes visible.

c Click again on the junction to continue wiring. d Click the end of the upper diode’s anode pin.

6 Continue connecting parts until the circuit is wired as

shown in Figure 2 on page 2-16.

To stop wiring, right-click and choose End Wire. The pointer changes to the default arrow.

Clicking on any valid connection poi nt ends a wire. A valid connection poin t is shown as

box

(see Figure 3).

Figure 3

If you make a mistake when placing or connecting components:

1 From the Edit menu, choose Undo, or

Connection points.

click .

To assign names (labels) to the nets

1 From the Place menu, choose Net Alias to display th e

Place Net Alias dialog box.

2 In the Name text box, type 3 Click OK. 4 Place the net alias on any segment of the wire that

connects R1, R2, R3, the diodes, and t he capacitor. The lower left corner of the net alias must touch the wire.

5 Right-click and choose En d Mode to quit the Net Alias

function.

Mid.

Chapter 2 Simulation examples

To assign names (labels) to the off-page connectors

Label the off-page connectors as shown in Figure 2 on page 2-16.

1 Double-click the name of an off-page connector to

display the Display Properties dialog box.

2 In the Name text box, type the new name. 3 Click OK. 4 Select and relocate the new name as desired.

To assign names to the parts

A more efficient way to change the names, values and other properties of several parts in your design is to use the Property Editor, as follows:

1 Select all of the parts to be modified

by pressing C and clicking each part.

2 From the Edit menu, choose

Properties. The Parts Spreadsheet appears. Change the entries in as many of the

cells as needed, and then click Apply to update all of the changes at once.

1 Double-click the second VDC part to display the Parts

spreadsheet.

2 Click in the first cell under the Reference column. 3 Type in the new name Vin. 4 Click Apply to update the changes to the part, then

close the spreadsheet.

5 Continue naming the remaining parts until your

schematic looks like Figure 2 on page 2-16.

To change the values of the parts

1 Double-click the voltage label (0V) on V1 to display

the Display Properties dialog box.

2 In the Value text box, type 3 Click OK. 4 Continue changing the Part Value properties of the

parts until all the parts are defined as in Figure 2 on page 2-16.

Your schematic page should now have the sam e parts, wiring, labels, and properties as Figure 2 on page 2-16.

5V.

pre

To save your design

1 From the File menu, choose Save.

Finding out more about setting up your design

About setting up a design for simulation

For a checklist of all of the things you need to do to se t up your design for simulation, and how to avoid common problems, see Chapte r 3,

Preparing a design for simulation.

Example circuit creation

Chapter 2 Simulation examples

Running PSpice

When you perform a simulation, PSpice generates an output file (*.OUT).

You can set up a simulation profile to run one analysis at a time. To run multiple analyses (for example, both DC sweep and transient analyses), set up a batch simulation. For more information, see

Chapte r 7,

and starting simulation.

Setting up analyses

While PSpice is running, the progress of the simulation appears and is updated in the PSpice simulation output window (see Figure 4).

Figure 4 PSpice simulation output window.

Performing a bias point analysis

To set up a bias point analysis in Capture

1 In Capture, switch to CLIPPER.OPJ in the schematic

page editor.

2 From the PSpice menu, choose New Simulation

Profile to display the New Simulation dialog box.

The root schematic listed is the schematic page associated with the simulation profile you are creating.

3 In the Name text box, type 4 From the Inherit From list, select None, then click

Create. The Simulation Settings dialog box appears.

5 From the Analysis type list, select Bias Point. 6 Click OK to close the Simulation Settings dialog box.

Bias.

To simulate the circuit from within Capture

1 From the PSpice menu, choose Run.

PSpice simulates the circuit and calculates the bias point information.

Running PSpice

Note

Because waveform data is not calculated during a bias point analysis, you will not see any plots displayed in the Probe window for this simulation. To find out how to view the results of this simulation, see

Using the simulation output file

below.

Chapter 2 Simulation examples

Using the simulation output file

The simulation output file acts as an audit trail of the simulation. This file optionally echoes the contents of the circuit file as well as the results of the bias point calculation. If there are any syntax errors in the netlist declarations or simulation commands, or a nomalies while performing the calculation, PSpice writes error or warning messages to the output file.

To view the simulation output file

1 From PSpice’s View menu, choose Output File.

Figure 5 shows the results of the bias point calc ulation as written in the simulation output file.

Figure 5 Simulation output file. 2 When finished, close the window.

PSpice measures the current through a two terminal device into the first terminal and out of the second terminal. For voltage sources, current is measur ed from the positive terminal to the negative terminal; this is opposite to the positive current flow convention and results in a negative value in the output file.

Finding out more about bias point calculations

Table 2-1

To find out more about this... See this...

Running PSpice

bias point calculations

Bias point on page 8-223

Chapter 2 Simulation examples

DC sweep analysis

You can visually verify the DC response of the cli pper by performing a DC sweep of the input voltage source and displaying the waveform results in the Probe window in PSpice. This example sets up DC sweep analysis parameters to sweep Vin from -10 to 15 volts in 1 volt increments.

Setting up and running a DC sweep analysis

To set up and run a DC sweep analysis

1 In Capture, from the PSpice menu, choose

New Simulation Profile. The New Simulation dialog box appears.

Note

The default settings for DC Sweep simulation are Voltage Source as the swept variable type and Linear as the sweep type. To use a different swept variable type or sweep type, choose different options under Sweep variable and Sweep type.

2 In the Name text box, type 3 From the Inherit From list, select Schematic1-Bias,

then click Create. The Simulation Settings dialog box appears.

4 Click the Analysis tab. 5 From the Analysis type list, select DC Sweep and enter

the values shown in Figure 6.

DC Sweep.

Figure 6 DC sweep analysis settings. 6 Click OK to close the Simulation Settings dialog box. 7 From the File menu, choose Save. 8 From the PSpice menu, choose Run to run the analysis.

DC sweep analysis

Chapter 2 Simulation examples

Displaying DC analysis results

Probe windows can appear during or after the simulation is finished.

press

press C+M

Figure 7 Probe window.

To plot voltages at nets In and Mid

1 From PSpice’s Trace menu, choose Add Trace. 2 In the Add Traces dialog box, select V(In) and V(Mid). 3 Click OK.

To display a trace using a marker

1 From Capture’s PSpice menu, point to Markers and

choose Voltage Level.

2 Click to place a marker on net Out, as shown in

Figure 8.

Figure 8 Clipper circuit with voltage marker on net Out. 3 Right-click and choose End Mode to stop placing

markers.

4 From the File menu, choose Save.

DC sweep analysis

5 Switch to PSpice. The V(Out) waveform trace appears,

as shown in Figure 9.

Figure 9 Voltage at In, Mid, and Out.

Chapter 2 Simulation examples

This example uses the cursors feature to view the numeric values for two traces an d the difference between them by placing a cursor on each trac e.

Table 10

Association of cursors with mouse

buttons.

cursor 1 left mouse button cursor 2 right mouse button

Figure 11

Trace legend with cursors

activated.

To place cursor s on V( In) and V(Mid)

1 From PSpice’s Trace menu, point to Cursor and

choose Display. Two cursors appear for the first trace defined in the

legend below the x-axis—V(In) in this example. The Probe Cursor window also appears.

2 To display the cursor crosshairs:

a Position the mouse anywhere inside the Probe

window.

b Click to display the crosshairs for the first cursor. c Right-click to display the crossha irs for the second

cursor.

In the trace legend, the part for V(I n) is outlined i n the crosshair pattern for each cursor, resulting in a dashed line as shown in Figure 11.

3 Place the first cursor on the V(In) waveform:

a Click the portion of the V(In) trace in the proximity

of 4 volts on the x-axis. The cursor crosshair appears, and the current X and Y values for the first cursor appear in the cursor window.

Your ability to get as close to 4.0 as possible depends on screen resolution and window size.

Figure 12

Trace legend with V(Mid)

symbol outlined.

b To fine-tune the cursor location to 4 volts on the

x-axis, drag the crosshairs until the x-axis value of the A1 cursor in the cursor window is approximately 4.0. You can also press r and l for tighter control.

4 Place the second cursor on the V(Mid) waveform:

a Right-click the trace legend part (diamond) for

V(Mid) to associate the second cursor with the Mid waveform. The crosshair pattern for the second cursor outlines the V(Mid) trace part as shown in Figure 12.

b Right-click the portion on the V(Mid) trace that is

in the proximity of 4 volts on the x-axis. The X and Y values for the second cursor appear in the cursor window along with the difference (dif) between the two cursors’ X and Y values.

c To fine-tu ne the location of the second cursor to 4

volts on the x-axis, drag the crosshairs until the x-axis value of the A2 cursor in the cursor window is approximately 4.0. You can also press V+r and V+l for tighter control.

DC sweep analysis

Figure 13 shows the Probe window with both cursors placed.

Figure 13 Voltage difference at V(In) = 4 volts.

To delete all of the traces

1 From the Trace menu, choose Delete All Traces.

At this point, the design has been saved. If needed, you can quit Capture and PSpice and complete the remaining analysis exercises later using the saved design.

There are also ways to display the difference between two voltages as a trac e:

• In PSpice, add the trace expression

V(In)-V(Mid).

• In Capture, from the PSpice menu,

point to Markers and choose Voltage Differential. Place the two markers on different pins or wires.

You can also delete an individual trace by selecting its name in the trace legend and then pressing D.

Example: To delete the V(In) trace, click the

V(In), located under the plot’s

text, x-axis, and then press D.

Finding out more about DC sweep analysis

Table 2-1

To find out more about this... See this...

DC sweep analysis

DC Sweep on page 8-214

Chapter 2 Simulation examples

Transient analysis

This example shows how to run a transient analysis on the clipper circuit. This requires adding a time-domain voltage stimulus as shown in Figure 14.

Figure 14 Diode clip per circuit wit h a voltage stimu lus.

To add a time-domain voltage stimulus

1 From Capture’s PSpice menu, point to Markers and

choose Delete All.

2 Select the ground part beneath the VIN source. 3 From the Edit menu, choose Cut. 4 Scroll down (or from the View menu, point to Zoom,

then choose Out).

5 Place a VSTIM part (from the PSpice library

SOURCESTM.OLB) as shown in Figure 14.

Transient analysis

6 From the Edit menu, choose Paste. 7 Place the ground part under the VSTIM part as shown

in Figure 14.

8 From the View menu, point to Zoom, then choose All. 9 From the File menu, choose Save to save the design.

To set up the stimulus

1 Select the VSTIM part (V3). 2 From the Edit menu, choose PSpice Stimulus.

The New Stimulus dialog box appears.

3 In the New Stimulus dialog box, type 4 Click SIN (sinusoidal), then click OK. 5 In the SIN Attributes dialog box, set the first three

properties as follows:

Offset Voltage = 0 Amplitude = 10 Frequency = 1kHz

6 Click Apply to view the waveform.

SINE.

or press C+v

Note

The Stimulus Editor is

not included in PSp ice Basics.

If you do not have the Stimulus Editor

1 Place a VSIN part instead of V STIM and

double-click it.

2 In the Edit Part dialog box, click User

Properties.

3 Set values for the VOFF, VA MPL, and

FREQ properties as defined in step 5 When finished, click OK.

The Stimulus Editor window should look like Figure 15.

Chapter 2 Simulation examples

Figure 15 Stimulus Editor window. 7 Click OK.

Figure 16

settings.

press V+@

Transient anal ysis simulation

8 From the File menu, choose Save to save the stimulus

information. Click Yes to update the schematic.

9 From the File menu, choose Exit to exit the Stimulus

Editor.

To set up and run the transient analysis

1 From Capture’s PSpice menu, choose

New Simulation Profile. The New Simulation dialog box appears.

2 In the Name text box, type 3 From the Inherit From list, select

Schematic1-DC Sweep, then click Create. The Simulation Settings dialog box appears.

4 Click the Analysis tab. 5 From the Analysis list, select Time Domain (Transient)

and enter the settings shown in Figure 16. TSTOP = 2ms Start saving data after = 20ns

Transient.

6 Click OK to close the Simulation Settings dialog box.

or press

7 From the PSpice menu, choose Run to perform the

analysis.

Transient analysis

PSpice uses its own internal time steps for computation. The internal time step is adjusted according to the requirements of the transient analysis as it proceeds. PSpice saves data to the waveform data file for each internal time step.

To display the input sine wave and clipped wave at V(Out)

1 From PSpice’s Trace menu, choose Add Trace. 2 In the trace list, select V(In) and V(Out) by clicking

them.

3 Click OK to display the traces. 4 From the Tools menu, choose Options to display the

Probe Options dialog box.

5 In the Use Symbols frame, click Always if it is not

already enabled.

6 Click OK.

Note

The internal time step is different from the Print Step value. Print Step controls how often optional text format data is written to the simula tion output file(*.OUT).

These waveforms illustrate the clipping of the input signal.

Figure 17 Sinusoidal input and clipped output waveforms.

Chapter 2 Simulation examples

Finding out more about transient analysis

Table 2-1

To find out more about this... See this...

transient analysis for analog designs*

* Includes how to set up time-based stimuli using the Stimulus Editor.

Chapter 10, Transient analysis

AC sweep analysis

The AC sweep analysis in PSpice is a linear (or small signal) frequency domain analysis that can be used to observe the frequency response of any circuit at its bias point.

Setting up and running an AC sweep analysis

In this example, you will set up the clipper circuit for AC analysis by adding an AC voltage source for a stimulus signal (see Figure 18) and by setting up AC sweep parameters.

AC sweep analysis

Figure 18 Clipper circuit with AC stimulus.

To change Vin to include th e AC stimulus signal

1 In Capture, open CLIPPER.OPJ. 2 Select the DC voltage source, Vin, and press D to

remove the part from the schematic page.

Chapter 2 Simulation examples

3 From the Place menu, choose Part.

Note

PSpice simulation is not case-sensitive, so both M and m can be used as “milli,” and MEG, M eg, an d meg c an all be used for “mega.” However, waveform analysis treats M and m as mega and milli, respectively.

4 In the Part text box, type

VAC (from the PSpice library

SOURCE.OLB) and click OK.

5 Place the AC voltage source on the schematic page, as

shown in Figure 17.

6 Double-click the VAC part (0V) to display the Parts

spreadsheet.

7 Change the Reference cell to Vin and change the

ACMAG cell to 1V

8 Click Apply to update the changes and then close the

spreadsheet.

To set up and run the AC sweep simulation

1 From Capture’s PSpice menu, choose New Simulation

Profile.

2 In the Name text box, enter AC Sweep, then click

create. The Simulation Settings dialog box appears.

3 Click the Analysis tab.

4 From the Analysis type list, select A C Sweep/Noise

and enter the settings shown in Figure 19.

Figure 19 AC sweep and noise analysis simulation settings.

5 Click OK to close the Simulation Settings dialog box.

6 From the PSpice menu, choose Run to start the

simulation. PSpice performs the AC analysis.

To add markers for waveform analysis

AC sweep analysis

1 From Capture’s PSpice menu, point to Markers, point

to Advanced, then choose db Magnitude of Voltage.

2 Place one Vdb marker on the Out net, then place

another on the Mid net.

3 From the File menu, choose Save to save the design.

AC sweep analysis results

PSpice displays the dB mag nitude (20log10) of th e voltage at the marked nets, Out and Mid, in a Probe window as shown in Figure 20 below. VDB(Mid) has a lowpass response due to the diode capacitances to ground. The output capacitance and load resistor act as a highpass filter, so the overall response, illustrated by VDB( out), is a bandpass response. Because AC is a linear analysis and the input voltage was set to 1V, the output voltage is the same as the gain (or attenuation) of the circu it.

ote

ou must first define a simulation profile for the AC Sweep/Noise analysis in order to use advanced markers.

Chapter 2 Simulation examples

Figure 20 dB magnitude curves for “gain” at Mid and Out.

To display a Bode plot of the output voltage, inc luding phase

Note

Depending upon where the Vphase marker was placed, the trace name may be different, such as VP(Cout:2), VP(R4:1), or VP(R4:2).

For more information on Probe windows and trace expressions, see C h a p t er 13,

Analyzing waveforms.

press C+x

press C+V

1 From Capture’s PSpice menu, point to Markers, point

to Advanced and choose Phase of Voltage.

2 Place a Vphase marker on the output next to the Vdb

marker.

3 Delete the Vdb marker on Mid. 4 Switch to PSpice.

In the Probe window, the gain and phase plots both appear on the same graph with the same scale.

5 Click the trace name VP(Out) to select the tr ace. 6 From the Edit menu, choose Cut. 7 From the Plot menu, choose Add Y Axis. 8 From the Edit menu, choose Paste.

The Bode plot appears, as shown in Figure 21.

Figure 21 Bode plot of clipper’s frequency response.

Finding out more about AC sweep and noiseanalysis

AC sweep analysis

Table 2-2

To find out more about this... See this...

AC sweep analysis

noise analysis based on an AC sweep analysis

AC sweep analysis on page 9-232

Noise analysis on page 9-241

Chapter 2 Simulation examples

Parametric Analysis is

Note

not supported in PS pice Basics.

Parametric analysis

This example shows the effect of varying input resistance on the bandwidth and gain of the clipper circuit by:

• Changing the value of R1 to the expression {Rval}.

• Placing a PARAM part to declare the parameter Rval.

• Setting up and running a parametric analysis to step

the value of R1 using Rval.

Figure 22 Clipper circuit with global parameter Rval.

This example produces multiple analysis runs, each with a different value of R1. After the analysis is complete, you can analyze curve families for the analysis runs using PSpice.

Setting up and running the parametric analysis

To change the value of R1 to the expression {Rval}

Parametric analysis

1 In Capture, open CLIPPER.OPJ. 2 Double-click the value (1k) of part R1 to display the

Display Properties dialog box.

3 In the Value text box, replace 1k with 4 Click OK.

{Rval}.

To add a PARAM part to declare the parameter Rval

1 From Capture’s Place menu, choose Part. 2 In the Part text box, type

library SPECIAL.OLB) , then click OK.

3 Place one PARAM part in any open area on the

schematic page.

4 Double-click the PARAM part to display the Parts

spreadsheet, then click New.

5 In the Property Name text box, enter Rval (no curly

braces), then click OK. This creates a new property for the PARAM part, as

shown by the new column labeled Rval in the spreadsheet.

PARAM (from the PSpice

PSpice interpret s t e xt in curly braces as an expression that evaluates to a numerical value. This example uses the simplest form of an expression—a constant. The value of R1 will take on the value of the Rval parameter, whatever it may be.

For more inf o rmation about using

Note

the Parts spreadsheet, see the OrCAD Capture User’s Guide.

6 Click in the cell below the Rval column and enter 1k

as the initial value of the parametric sweep.

7 While this cell is still selected, click Display. 8 In the Display Format frame, select Name and Value,

then click OK.

9 Click Apply to update all the changes to the PARAM

part.

10 Close the Parts spreadsheet. 11 Select the VP marker and press

marker from the schematic page.

12 From the File menu, choose Save to save the design.

D to remove the

This example is only interested in the magnitude of the response.

Chapter 2 Simulation examples

To set up and run a parametric analysis to step the value of R1 using Rval

1 From Capture’s PSpice menu, choose

New Simulation Profile. The New Simulation dialog box appears.

The root schematic listed is the schematic page associated with the simulation profile you are creating.

This profile specifies that the parameter Rval is to be stepped from 100 to 10k logarithmically with a resolution of 10 points per decade.

The analysis is run for each value of Rval. Because the value of R1 is defined as {Rval}, the analysis is run for each v alue of R1 as it logarit hm ically increases from

Ω to 10 kΩ in 20 steps, resulting in a

100 total of 21 runs.

2 In the Name text box, type

Parametric.

3 From the Inherit From list, select AC Sweep, then clic k

Create. The Simulation Settings dialog box appears.

4 Click the Analysis tab. 5 Under Options, select Parametric Sweep and enter the

settings as shown below.

Figure 23 Parametric simulation settings. 6 Click OK. 7 From the PSpice menu, choose Run to start the

analysis.

Analyzing waveform families

Continuing from the example above, there are 21 analysis runs, each with a different value of R1. After PSpice completes the simulation, the Available Sections dialog box appears, listing all 21 runs and the Rval parameter value for each. You can select one or more runs to display.

To display all 21 traces

Parametric analysis

1 In the Available Sections dialog box, click OK.

All 21 traces (the entire family of curves) for VDB(Out) appear in the Probe window as shown in Figure 24.

Figure 24 Small signal response as R1 is varied from 100

Ω

to 10 k

2 Click the trace name to select it, then press D to

remove the traces shown.

Ω

To select individual runs, click each one separately.

To see more information about the section that produced a speci fic t race, double-click the corresponding symbol in the legend below the x-ax is.

You can also remove the traces by removing the VDB marker from your schematic page in Capture.

Chapter 2 Simulation examples

press I

To compare the last run to the first run

1 From the Trace menu, choose Add Trace to display the

Add Traces dialog box.

2 In the Trace Expression text box, type the following:

You can avoid some of the typing for the Trace Expression text box by selecting V(OUT) twice in the trace list and inserting text where appropriate in the resulting Trace Expression.

press I

Vdb(Out)@1 Vdb(Out)@21

3 Click OK.

Note

The difference in gain is apparent. You can also plot the difference of the waveforms for runs 21 and 1, then use the search commands to find certain characteristics of the difference.

4 Plot the new trace by specifying a waveform

expression:

a From the Trace menu, choose Add Trace. b In the Trace Expression text box, type the

following waveform expression:

Vdb(Out)@1-Vdb(OUT)@21

c Click OK.

5 Use the search commands to find the value of the

difference trace at its maximum and at a specific frequency:

a From the Tools menu, point to Cursor and choose

Display.

b Right-click then left-click the trace part (triangle)

for Vdb(Out)@1 - Vdb(Out)@21. Make sure that you left-click last to make cursor 1 the active cursor.

The search command tells PSpice to search for the point on the trace where the x-axis value is 100.

c From the Trace menu, point to Cursor and choose

Max.

d From the Trace menu, point to Cursor and choose

Search Commands.

e In the Search Command text box, type the

following:

search forward x value (100)

f Select 2 as the Cursor to Move option.

g Click OK.

Figure 25 shows the Probe window with cursors placed.

Figure 25 Small signal frequen cy response at 100 and 10 kΩ

input resistance.

Parametric analysis

Note that the Y value for cursor 2 in the cursor box is about 17.87. This indicat es that when R1 is set to 10 k the small signal attenuation of the circuit at 100Hz is

17.87dB greater than when R1 is 100

Ω.

6 From the Trace menu, point to Cursor and choose

Display to turn off the display of the cursors.

7 Delete the trace.

Ω,

Chapter 2 Simulation examples

Finding out more about parametric analysis

Table 2-3

To find out more about this... See this...

parametric analysis

using global parameters Using global parameters and

Parametric analysis on page 11-272

expressions for values on page 3-67

Performance analysis

Performance analysis is an advanced feature in PSpice that you can use to compare the characteristics of a family of waveforms. Performance analysis uses the principle of search commands introduced earlier in this chapter to define functions that detect points on each curve in the family.

After you define these functions, you can apply them to a family of waveforms and produce traces that are a function of the variable that changed within the family.

This example shows how to use performance analysis to view the dependence of circuit characteristics on a swept parameter. In this case, the small signal bandwidth and gain of the clipper circuit are plotted against the swept input resistance value.

To plot bandwidth vs. Rval using the performance analysis wizard

1 In Capture, open CLIPPER.OPJ.

Performance analysis

2 From PSpice’s Trace menu, choose Performance

Analysis. The Performance Analysis dialog box appears with

information about the currently loaded data and performance analysis in general.

3 Click the Wizard button. 4 Click the Next> button. 5 In the Choose a Goal Function list, click Bandwidth,

then click the Next> button.

6 Click in the Name of Trace to search t ext box and type

V(Out).

7 Click in the db level down for bandwidth calc text box

and type

8 Click the Next> button.

The wizard displays the gain trace for the first run (R=100) and shows how the bandwidth is measured. This is done to test the goal function.

At each step, the wizard provides information and guidelines.

Click , then double-click V(Out).

Chapter 2 Simulation examples

9 Click the Next> button or the Finish button.

A plot of the 3dB bandwidth vs. Rval appears.

10 Change the x-axis to log scale:

Double-click the x-axis.

or press I

The Trace list in cludes goal f unctions on ly in performance analysis mode when the x-axis variable is the swept parameter.

a From the Plot menu, choose Axis Settings. b Click the X Axis tab. c Under Scale, choose Log. d Click OK.

To plot gain vs. Rval manually

1 From the Plot menu, choose Add Y Axis. 2 From the Trace menu, choose Add to display the Add

Traces dialog box.

3 In the Functions or Macros frame, select the Goal

Functions list, and then click the Max(1) goal function.

4 In the Simulation Output Variables list, click V(out). 5 In the Trace Expression text box, edit the text to be

Max(Vdb(out)), then click OK.

PSpice displays gain on the second y-axis vs. Rval.

Figure 26 shows the final performance analysis plot of 3dB bandwidth and gain in dB vs. the swept input resistance value.

Figure 26 Performance analysis plots of bandwidth and gain vs.

Rval.

Finding out more about performance analysis

Table 2-4

To find out more about this... See this...

Performance analysis

how to use performance analysis

how to use search commands and create goal functions

RLC filter example on page 11-274

Example: Monte Carlo analysis of a pressure sens or on page 12-293

PSpice A/D online Help

Chapter 2 Simulation examples

Part two

Design entry

Part two provides information about how to enter circuit designs in OrCAD

• Chapter 3, Preparing a desi gn for simul ation, outlines the

things you need to do to successfully simulate your schematic including troubleshooting tips for the most frequently asked questions.

• Chapter 4, Creating and editing models, describes how to

use the tools to create and edit model definitions, and how to configure the models for use.

• Chapte r 5, Creating parts for models, explains how to

create symbols for existing or new model definitions so you can use the models when simulating from your schematic.

•

Chapter 6, Analog behavioral modeli ng, describes how to

model analog behavior mathe mati call y or using table lookups.

Capture that you want to simulate.

Preparing a design for simulation

Chapter overview

This chapter provides introductory information to help you enter circuit designs that simulate properly. If you want an overview, use the checklist on page 3-56 you to specific topics.

Topics include:

•

Checklist for simulation setup on page 3-56

• Using parts that you can simulate on page 3-60

•

Using global parameters and expressions for values on page 3-67

•

Defining power supplies on page 3-74

•

Defining stimuli on page 3-75

•

Things to watch for on page 3-79

to guide

Refer to your OrCAD Capture User’s Guide for ge neral schematic

entry information.

Chapter 3 Preparing a design for simulation

Checklist for simulation setup

This section describes what you need to do to set up your circuit for simulation.

1 Find the topic that is of interest in the first column of

any of these tables.

2 Go to the referenced section. For those sections that

provide overviews, you will find references to more detailed discussions.

Typical simulation setup steps

For more information on this step... See this... To find out this...

Set component values

✔

and other properties.

Define power

✔

supplies. Define input

✔

waveforms. Set up one or more

✔

analyses.

Using parts that you can simulate on page 3-60

Using global parameters an d expressions for values on page 3-67

Defining power supplies on page 3-74

Defining stimuli on page 3-75

Chapter 7, Setting up analyses and starting simulation

Chapter 8 Chapter 12

contents)

through

(see the table of

An overview of vendor, passive, breakout, and behavioral parts.

How to define values using variable parameters, functional calls, and mathematical expressions.

An overview of DC power for analog circuits..

An overview of DC, AC, and time-based stimulus parts.

Procedures, general to all analysis types, to set up and start the simulation.

Detailed information about DC, AC, transient, parametric, temperature, Monte Carlo, and sensitivity/worst-case..

For more information on this step... See this...

Checklist for simulation setup

Place markers. Using schematic page

✔

markers to add traces on

How to display results in PSpice by picking design nets.

page 13-331

✔

Limiting waveform data file

How to limit the data file size.

size on page 13-334

Advanced design entry and simulation setup steps

For more information on this step... See this... To find out how to...

Create new models. Chapter 4, Creating and

✔

editing models

Chapter 6, Analog behavioral modeling

Create new parts. Chapter 5, Creating parts

✔

for models

Define models using the Model Editor or Create Subcircuit command.

Define the behavior of a block of analog circuitry as a mathematical function or lookup table.

Create parts either automatically for models using the part wizard or the Parts utility, or by manually defining AKO parts; define simulation-specific properties.

OrCAD Capture User’s

The

Guide

Create and edit part graphics, pins, and properties in general.

Chapter 3 Preparing a design for simulation

When netlisting fails or the simulation does not start

If you have problems starting the simulation, there may be problems with the design or with system resources. If there are problems with the design, PSpice displays errors and warnings in the Simulation Output window. You can use the Simulation Output window to get more information quickly about the specific problem.

To get online info rmation ab out an e rror or w arning sh own in the Simulation Output window

1 Select the error or warning message. 2 Press 1.

The following tables list the most commonly encountered problems and where to find out more about what to do.

Things to check in your design

Table 5

Make sure that... To find out more, see this...

The model libraries, stimulus files, and

✔

include files are configured. The parts you are using have models.

✔

You are not using unmodeled pins.

✔

You have defined the grounds.

✔

Every analog net has a DC path to ground.

✔

The part template is correct.

✔

Hierarchical parts, if used, are properly

✔

defined. Ports that connect to the same net have the

✔

same name.

Configuring model libraries on page 4-120

Unmodeled parts on page 3-79 properties needed for simulation on page 5-139

Unmodeled pins on page 3-82 Missing ground on page 3-83 Missing DC path to ground on page 3-84 Defining part properties needed for simulation on

page 5-139

The

OrCAD Capture User’s Guide

The

OrCAD Capture User’s Guide

and

Defining part

Things to check in your system configuration

Table 6

Make sure that... To find out more, see this...

Path to the PSpice programs is correct.

✔

Checklist for simulation setup

Directory containing your design has write

✔

permission. Your system has sufficient free memory

✔

and disk space.

Your operating system manual

Chapter 3 Preparing a design for simulation

Using parts that you can simulate

The OrCAD part libraries also include special parts that you can use for simulation only. These inclu de:

• stimulus parts

input signals to the circuit (see

Defining stimuli page 3-75

• ground parts

analog circuits, which need reference to ground

• simulation control parts

to do things like set bias values (see

Appendix A,

state

• output control parts

things like generate tables and line-printer plots to th e PSpice output file (see

output options

)

Chapter 14,

to generate

required by all

Setting initial

to do

Other

)

The OrCAD part libraries supply numerous parts designed for simulation. These include:

• vendor-supplied parts

• passive parts

• breakout parts

• behavioral parts

At minimum, a part that you can simulate has these properties:

• A simulation model to describe the part’s electrical

behavior; the mo del can be:

• explicitly defined in a model library,

• built into PSpice, or

• built into the part (for some kinds of analog

behavioral parts).

• A part with modeled pins to form electrical

connections in your design.

• A translation from design part to netlist statement so

that PSpice can read it in.

Note

Not all parts in the libraries are set up for simulation. For example, connectors are parts destined for board layout only and do not have these simulation properties.

Vendor-supplied parts

Using parts that you can simulate

The OrCAD libraries provide an extensive selection of manufacturers’ analog parts. Typically, the library name reflects the kind of parts contained in the library and the vendor that provided the models.

Example: MOTOR_RF.OLB and MOTOR_RF.LIB contain parts and models, respectively, for Motorola-made RF bipolar transistors.

Part naming conventions

The part names in the OrCAD libraries usually reflect the manufacturers’ part names. If multiple vendors supply the same part, each part name includes a suffix that indicates the vendor that supplied the model.

Example: The OrCAD libraries include several models for the OP-27 opamp as shown by these entries in the online Library List.

For a listing of vendor-supplied parts contained in the OrCAD libraries, refer to the online Library List.

To find out more about each model library, read the comments in the .LIB file header.

Chapter 3 Preparing a design for simulation

Notice the following:

• There is a generic OP-27 part provided by OrCAD, the

OP-27/AD from Analog Devices, Inc., and the OP-27/LT from Linear Technology Corporation.

• The Model column for all of these parts contains an

asterisk. This indicates that this part is modeled and that you can simulate it.

Finding the part that you want

If you are having trouble finding a part, you can search the libraries for parts with similar names by using either:

• the parts browser in Capture and restricting the parts

list to those names that match a specified wildcard text string, or

• the online Library List and searching for the generic

part name using capabilities of the Adobe Acrobat Reader.

Note

This method finds any part contained in the current part libraries configuration, including parts for user-defined models.

If you want to find out more about a part supplied in the OrCAD libraries, such as manufacturer or whether you can simulate it, then search the online Library List (see page3-63

To find parts using the parts browser

1 In Capture, from the Place menu, choose Part. 2 In the Part Name text box, type a text string with

wildcards that approximates the part name that you want to find. Use this syntax:

where <wildcard> is one of the following: * to match zero or more characters

? to match exactly one character The parts browser displays only the matching part

names.

Using parts that you can simulate

or press C+F

To find parts using the online OrCAD Library List

1 In Windows Explorer, double-click LIBLIST.PDF,

located in the directory where PSpice is installed. Acrobat Reader starts and displays the OrCAD

Library List.

2 From the Tools menu, choose Find. 3 In the Find What text box, type the generic part name. 4 Enter any other search criteria, and then click Find.

The Acrobat Reader displays the first page where it finds a match. Each page maps the generic part name to the parts (and corresponding vendor and part library name) in the OrCAD libraries.

5 If you want to repeat the search, from the Tools menu,

choose Find Again.

Note

If you are unsure of the device type, you can scan all of the device type lists using the Acrobat search capability. The first time you do this, you need to set up the across-list index. To find out more, refer to the online Adobe Acrobat manuals.

Note

This method finds only parts that

OrCAD supplies that have models.

If you want to include user-defined parts in the search, use the parts browser in Capture (see page 3-62

Instead of the generic part name, you can enter other kinds of search information, such as device type or manufacturer.

press C+G

Chapter 3 Preparing a design for simulation

Passive parts

The OrCAD libraries supply several basic parts based on the passive device models built into PSpice. These are summarized in the following table.

Table 7 Passive parts

To find out more about how to use these parts and define their pr operties, look up the corresponding PSpice device letter in the Analog Devices chapter in the online OrCAD PSpice A/D

eference Manual, and then see the

Parts sections.

Capture

These parts are available... For this device t y pe ...

C C_VAR

Linductor L R

R_VAR XFRM_LINEAR

K_LINEAR T ideal transmission line T TLOSSY Lossy transmission line T

COUPLED*

COUPLEDX**

KCOUPLE

* For these device types, t he OrCAD libraries supply several parts. Refer to the

online parts.

OrCAD PSpice A/D Reference Manual

capacitor C

resistor R

transformer K and L

coupled transmission line T and K

Which is this PSpice device letter...

for the available

Breakout parts

The OrCAD libraries supply passive and semiconductor parts with default model definitions that define a basic set of model parameters. This way, you can easily:

Using parts that you can simulate

To find out more about models, see What

are models? on page 4-87

• assign device and lot tolerances to model parameters

for Monte Carlo and sensitivity/worst-case analyses,

• define temperature coefficients, and

• define device-specific operating temp eratures.

These are called breakout parts and are summarized in the following table.

Table 8 Breakout parts

Use this breakout part. .. For t h is device type...

BBREAK GaAsFET B CBREAK capacitor C DBREAK JBREAK KBREAK ind u ct o r coupling K LBREAK inductor L MBREAK QBREAK RBREAK resistor R

*JFET J

* MOSFET M

diode D

bipolar transistor Q

Which is this PS pice device letter...

To find out more about Monte Carlo and sensitivity/worst-case analyses, see

Chapter 12,

sensitivity/worst-ca se analyses

Monte Carlo and

To find out more about setting temperature parameters, see the Analog Devices chapter in the online OrCAD PSpice

/D Reference Manua l and find the

device type that you are interested in.

To find out more about how to use these parts and define their pr operties, look up the corresponding PSpice device letter in the Analog Devices chapter of the online OrCAD PSpice A/D

eference Manual, and then look in

the Capture Parts section.

SBREAK voltage-controlled

switch TBREAK transmission line T WBREAK current-controlled

switch XFRM_NONLINEAR transformer K and L ZBREAKN IGBT Z

* For this device type, the OrCAD libraries supply several breakout parts. Refer

to the onli ne parts.

OrCAD PSpice Ref e rence Manual

for the available

Chapter 3 Preparing a design for simulation

Behavioral parts

Behavioral parts allow you to define how a block of circuitry should work without having to define each discrete component.

For more information, see Chapte r 6,

Analog behavioral modeling

Analog behavioral parts

behavioral modeling (ABM) to define each part’s behavior as a mathematical expression or lookup table. The OrCAD libraries provide ABM parts that operate as math functions, limiters, Chebyshev filters, integrators, differentiators, and others that you can customize for specific expressions and lookup table s. You can also create your own ABM parts.

These parts use analog

Using global parameters and expressions for values

In addition to literal values, you can use global parameters and expressions to represent numeric values in your circuit design.

Global parameters

Using global parameters and expressions for values

A global parameter is like a programming variable that represents a numeric value by name.

Once you have defined a parameter (declared its name and given it a value), you can use it to represent circuit values anywhere in the design; this applies to any hierarchical level.

Some ways that you can use parameters are as follows:

• Apply the same value to multiple part instances.

• Set up an analysis that sweeps a var iable throu gh a

range of values (for example, DC sweep or parametric analysis).

Declaring and using a global parameter

To use a global parameter in your design, you need to:

• define the parameter using a PARAM part, and

•

use the parameter in place of a literal value somewhere in your design.

When multiple parts are set to the same value, glob al parameters pr ovide a convenient way to change all of their values for “what-i f ” analyses.

Example: If two independent so urces have a value defined by the parameter VSUPPLY, then you can change both sources to 10 volts by assi gning the value once to VSUPPLY.

Chapter 3 Preparing a design for simulation

To declare a g l ob al parameter

1 Place a PARAM part in your design.

Note

For more inf o rmation about using the Parts spreadsheet, see the OrCAD Capture User’s Guide.

Example: To declare the global parameter VSUPPLY that will set the value of an independent voltage source to 1 4 volts, place the PARAM part, and then create a new property named

14v

value of

VSUPPLY

with a

2 Double-click the PARAM part to display the Parts

spreadsheet, then click New.

3 Declare up to three global parameters by doing the

following for each global parameter:

a Click New. b In the Property Name text box, enter NAMEn, then

click OK. This creates a new property for the PARAM part,

NAMEn in the spreadsheet.

c Click in the cell below the NAMEn column and

enter a default value for the parameter.

d While this cell is still selected, click Display. e In the Display Format frame, select Name and

Value, then click OK.

Note

The system variables in

T a ble 11 on p age 3-73

have reserved parameter names. Do not use these parameter names when defining your own parameters.

4 Click Apply to update all the changes to the PARAM

part.

Example: To set the independent voltage source, VCC, to the value of the VSUPPLY parameter, set its DC property to

{VSUPPLY}

5 Close the Parts spreadsheet.

To use the global parameter in your circuit

1 Find the numeric value that you want to replace: a

component value, model parameter value, or other property value.

2 Replace the value with the name of the global

parameter using the following syntax: { global_parameter_name } The curly braces tell PSpice to evaluate the parameter

and use its value.

Orcad PSPICE User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Contents

Before you begin

Welcome to OrCAD

OrCAD PSpice overview

How to use this guide

Typographical conventions

Related documentation

Online Help

What’s New

Things you need to know

Chapter overview

What is PSpice?

Analyses you can run wi th PSpice

Basic analyses

Advanced multi-run analyses

Analyzing waveforms with PSpice

What is waveform analysis?

Using PSpice with other OrCAD programs

Using Capture to prepare for simulation

What is the Stimulus Editor?

What is the Model Editor?

Files needed for simulation

Files that Capture generates

Other files that you can configure for simulation

Files that PSpice generates

Simulation examples

Chapter overview

Example circuit creation

Finding out more about setting up your design

Running PSpice

Performing a bias point analysis

Using the simulation output file

Finding out more about bias point calculations

DC sweep analysis

Setting up and running a DC sweep analysis

Displaying DC analysis results

Finding out more about DC sweep analysis

Transient analysis

Finding out more about transient analysis

AC sweep analysis

Setting up and running an AC sweep analysis

AC sweep analysis results

Parametric analysis

Setting up and running the parametric analysis

Analyzing waveform families

Finding out more about parametric analysis

Performance analysis

Finding out more about performance analysis

Preparing a design for simulation

Chapter overview

Checklist for simulation setup

Typical simulation setup steps

Advanced design entry and simulation setup steps

When netlisting fails or the simulation does not start

Using parts that you can simulate

Vendor-supplied parts

Passive parts

Breakout parts

Behavioral parts

Using global parameters and expressions for values

Global parameters