PSpice® User's Guide

PSpice® User’s Guide
includes PSpice A/D, PSpice A/D Basics, and PSpice
Product Version 10.5
July 2005
 1985-2005 Cadence Design Systems, Inc. All rights reserved.
Printed in the United States of America.
Cadence Design Systems, Inc., 555 River Oaks Parkway, San Jose, CA 95134, USA
Trademarks: Trademarks and service marks of Cadence Design Systems, Inc. (Cadence)
contained in this document are attributed to Cadence with the appropriate symbol. For queries
regarding Cadence’s trademarks, contact the corporate legal department at the address shown
above or call 1-800-862-4522.
All other trademarks are the property of their respective holders.
Restricted Print Permission: This publication is protected by copyright and any unauthorized use
of this publication may violate copyright, trademark, and other laws. Except as specified in this
permission statement, this publication may not be copied, reproduced, modified, published,
uploaded, posted, transmitted, or distributed in any way, without prior written permission from
Cadence. This statement grants you permission to print one (1) hard copy of this publication subject
to the following conditions:
1
The publication may be used solely for personal, informational, and noncommercial purposes;
2
The publication may not be modified in any way;
3
Any copy of the publication or portion thereof must include all original copyright, trademark, and
other proprietary notices and this permission statement; and
4
Cadence reserves the right to revoke this authorization at any time, and any such use shall be
discontinued immediately upon written notice from Cadence.
Disclaimer: Information in this publication is subject to change without notice and does not
represent a commitment on the part of Cadence. The information contained herein is the proprietary
and confidential information of Cadence or its licensors, and is supplied subject to, and may be used
only by Cadence’s customer in accordance with, a written agreement between Cadence and its
customer. Except as may be explicitly set forth in such agreement, Cadence does not make, and
expressly disclaims, any representations or warranties as to the completeness, accuracy or
usefulness of the information contained in this document. Cadence does not warrant that use of such
information will not infringe any third party rights, nor does Cadence assume any liability for
damages or costs of any kind that may result from use of such information.
Restricted Rights: Use, duplication, or disclosure by the Government is subject to restrictions as
set forth in FAR52.227-14 and DFAR252.227-7013 et seq. or its successor.
PSpice User's Guide
Contents
Before you begin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
Welcome . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
How to use this guide . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Symbols and conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Related documentation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What this user’s guide covers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice A/D overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice A/D Basics overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Add-on options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice Smoke Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice Advanced Optimizer Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice Advanced Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
If you don’t have the standard PSpice A/D package . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Comparison of the different versions of PSpice . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
If you have PSpice A/D Lite . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum hardware requirements for running PSpice: . . . . . . . . . . . . . . . . . . . . . . . .
Part one: Simulation primer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
20
20
21
24
24
25
25
25
25
26
26
26
26
30
30
33
1
Things you need to know . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What is PSpice A/D? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analyses you can run with PSpice A/D . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Basic analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Advanced multi-run analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analyzing waveforms with PSpice . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What is waveform analysis? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using PSpice with other programs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using OrCAD Capture to prepare for simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What is the PSpice Stimulus Editor? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
3
35
36
40
40
43
45
45
46
46
46
Product Version 10.5
PSpice User's Guide
What is the PSpice Model Editor? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47
Files needed for simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47
Files that OrCAD Capture generates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48
Other files that you can configure for simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50
Files that PSpice generates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53
New directory structure for analog projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55
How are files configured at the design level maintained in the new directory structure for
analog projects? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58
How are files configured at the profile level maintained in the new directory structure for
analog projects? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60
What happens when I convert an analog project that uses a design from another project
or from another location? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62
What should I do if the schematic for a converted analog project uses FILESTIMn parts
from the SOURCE library? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62
2
Simulation examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63
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 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Finding out more about AC sweep and noise analysis . . . . . . . . . . . . . . . . . . . . . . . .
Parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up and running the parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
4
63
64
72
72
73
75
76
76
76
78
83
83
87
88
88
90
92
93
94
Product Version 10.5
PSpice User's Guide
Analyzing waveform families . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97
Finding out more about parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100
Performance analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101
Finding out more about performance analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103
Part two: Design entry
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105
3
Preparing a design for simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107
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 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Specifying values for part properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using global parameters and expressions for values . . . . . . . . . . . . . . . . . . . . . . . . . .
Global parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining power supplies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
For the analog portion of your circuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
For A/D interfaces in mixed-signal circuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analog stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Digital stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Things to watch for . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Unmodeled parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Unconfigured model, stimulus, or include files . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Unmodeled pins . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Missing ground . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Missing DC path to ground . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
5
107
108
108
109
110
111
112
117
118
120
120
121
121
124
133
133
133
135
135
138
140
140
144
145
146
146
Product Version 10.5
PSpice User's Guide
4
Creating and editing models
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What are models? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
How are models organized? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Model libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Model library configuration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Global vs. design vs. profile models and libraries . . . . . . . . . . . . . . . . . . . . . . . . . .
Nested model libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSpice-provided models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Model library data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Device characteristic curves-based models vs. Template-based models . . . . . . . .
Tools to create and edit models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ways to create and edit models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ways to use the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Running the Model Editor alone . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating models using the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating models based on device characteristic curves . . . . . . . . . . . . . . . . . . . . .
Creating models based on PSpice templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Importing an existing model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Enabling and disabling automatic part creation . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Running the Model Editor from the schematic editor . . . . . . . . . . . . . . . . . . . . . . . .
Model creation examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example: Creating a PSpice model based on device characteristic curves . . . . . . .
Example: Creating template-based PSpice model . . . . . . . . . . . . . . . . . . . . . . . . . .
Editing model text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example: editing a Q2N2222 instance model . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the Create Subcircuit Format Netlist command . . . . . . . . . . . . . . . . . . . . . . . . . .
Changing the model reference to an existing model definition . . . . . . . . . . . . . . . . . . .
Reusing instance models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Reusing instance models in the same schematic . . . . . . . . . . . . . . . . . . . . . . . . . .
Making instance models available to all designs . . . . . . . . . . . . . . . . . . . . . . . . . . .
Configuring model libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
6
149
151
152
152
153
153
154
155
155
157
160
161
163
164
165
166
166
166
171
174
175
177
180
180
187
193
195
196
199
200
200
201
202
Product Version 10.5
PSpice User's Guide
The Configuration Files tab . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 202
How PSpice uses model libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 203
Adding model libraries to the configuration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 205
Changing the model library scope from profile to design, profile to global, design to global
and vice versa . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 206
Changing model library search order . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 208
Changing the library search path . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 210
Handling smoke information using the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . 212
Adding smoke information to PSpice models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 212
Creating template-based PSpice models with smoke information . . . . . . . . . . . . . . 214
Using the Model Editor to edit smoke information . . . . . . . . . . . . . . . . . . . . . . . . . . 214
Examples: Smoke . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 215
Adding smoke information to the D1 diode model . . . . . . . . . . . . . . . . . . . . . . . . . . 215
Adding smoke information to the OPA_LOCAL operational amplifier model . . . . . . 216
Smoke parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 218
Diode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 219
Bipolar Junction Transistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 220
Magnetic Core . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 221
Ins Gate Bipolar Transistor (IGBT) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 222
Junction FET . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 223
Operational Amplifier . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 224
MOSFET . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 226
Voltage Regulator . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 228
Darlington Transistor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 229
5
Creating parts for models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 231
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What’s different about parts used for simulation? . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ways to create parts for models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Preparing your models for part creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting the Model Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the Model Editor to create parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Batch mode of part creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Interactive mode of part creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
7
231
232
233
235
236
237
237
237
Product Version 10.5
PSpice User's Guide
Creating Capture parts for all models in a library . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using batch mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using interactive mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up automatic part creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating parts in the batch mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating parts using interactive mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Basing new parts on a custom set of parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Editing part graphics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
How Capture places parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining grid spacing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Attaching models to parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
MODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining part properties needed for simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSPICETEMPLATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
IO_LEVEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
MNTYMXDLY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PSPICEDEFAULTNET . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
238
238
240
245
246
246
250
254
256
256
258
259
260
262
263
272
273
274
6
Analog behavioral modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 275
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of analog behavioral modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
The ABM.OLB part library file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Placing and specifying ABM parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Net names and device names in ABM expressions . . . . . . . . . . . . . . . . . . . . . . . . .
Forcing the use of a global definition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
ABM part templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Control system parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Basic components . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Limiters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Chebyshev filters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Integrator and differentiator . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Table look-up parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Laplace transform part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
8
275
276
277
278
278
279
280
281
284
285
286
290
291
296
Product Version 10.5
PSpice User's Guide
Math functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
ABM expression parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
An instantaneous device example: modeling a triode . . . . . . . . . . . . . . . . . . . . . . .
PSpice-equivalent parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Implementation of PSpice-equivalent parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Modeling mathematical or instantaneous relationships . . . . . . . . . . . . . . . . . . . . . .
Lookup tables (ETABLE and GTABLE) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency-domain device models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Laplace transforms (LAPLACE) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency response tables (EFREQ and GFREQ) . . . . . . . . . . . . . . . . . . . . . . . . .
Cautions and recommendations for simulation and analysis . . . . . . . . . . . . . . . . . . . . .
Instantaneous device modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency-domain parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Laplace transforms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Trading off computer resources for accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Basic controlled sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating custom ABM parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7
Digital device modeling
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 329
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Functional behavior . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Timing characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Timing model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Propagation delay calculation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Inertial and transport delay . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Input/Output characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Input/Output model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining Output Strengths . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Charge storage nets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating your own interface subcircuits for
additional technologies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating a digital model using the PINDLY and LOGICEXP primitives . . . . . . . . . . . . .
Digital primitives . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
299
299
303
307
308
309
313
315
315
317
320
320
321
322
325
326
326
9
329
330
331
339
339
342
343
346
346
350
352
353
358
359
Product Version 10.5
PSpice User's Guide
Logic expression (LOGICEXP primitive) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pin-to-pin delay (PINDLY primitive) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
BOOLEAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PINDLY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Constraint checker (CONSTRAINT primitive) . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setup_Hold . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Width . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Freq . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
74160 example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
359
361
362
363
364
365
365
366
366
Part three: Setting up and running analyses . . . . . . . . . . . . . . . . . 369
8
Setting up analyses and starting simulation . . . . . . . . . . . . . . . . . . 371
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analysis types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Execution order for standard analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Output variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Performance package . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting a simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating a simulation netlist . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting a simulation from Capture . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting a simulation outside of Capture . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up batch simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
The PSpice simulation window . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Interacting with a simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Extending a transient analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Interrupting a simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Scheduling changes to runtime parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the Simulation Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of the Simulation Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up multiple simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting, stopping, and pausing simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Attaching PSpice to a simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
10
371
372
373
374
376
383
385
385
394
394
395
396
400
401
404
406
409
409
413
414
415
Product Version 10.5
PSpice User's Guide
Setting options in the Simulation Manager . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 415
9
DC analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 419
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
DC Sweep . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a DC sweep analysis . . . . . . . . . . . . . . . . . . . . . . . .
Overview of DC sweep . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up a DC stimulus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Nested DC sweeps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Curve families for DC sweeps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a bias point analysis . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Small-signal DC transfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a small-signal DC transfer analysis . . . . . . . . . . . . .
Overview of small-signal DC transfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
DC sensitivity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a DC sensitivity analysis . . . . . . . . . . . . . . . . . . . . . .
Overview of DC sensitivity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
419
420
420
421
423
424
426
429
429
429
431
431
432
434
434
435
10
AC analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 437
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
AC sweep analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up and running an AC sweep . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What is AC sweep? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up an AC stimulus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up an AC analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
AC sweep setup in example.opj . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
How PSpice treats nonlinear devices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Noise analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up and running a noise analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What is noise analysis? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up a noise analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
11
437
438
438
438
439
442
444
446
448
448
449
450
Product Version 10.5
PSpice User's Guide
Analyzing Noise in the Probe window
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 452
11
Parametric and temperature analysis . . . . . . . . . . . . . . . . . . . . . . . . . 457
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a parametric analysis . . . . . . . . . . . . . . . . . . . . . . . .
Overview of parametric analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
RLC filter example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example: frequency response vs. arbitrary parameter . . . . . . . . . . . . . . . . . . . . . . .
Temperature analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a temperature analysis . . . . . . . . . . . . . . . . . . . . . . .
Overview of temperature analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
457
458
458
459
459
464
467
467
468
12
Transient analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 471
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of transient analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum requirements to run a transient analysis . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining a time-based stimulus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of stimulus generation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
The Stimulus Editor utility . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Stimulus files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Configuring stimulus files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting the Stimulus Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating new stimulus symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Editing a stimulus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Deleting and removing traces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Manual stimulus configuration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Finding out more about the Stimulus Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Transient (time) response . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Internal time steps in transient analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Switching circuits in transient analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Plotting hysteresis curves . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
12
471
472
472
474
474
476
477
477
478
478
483
484
485
485
487
487
490
491
492
Product Version 10.5
PSpice User's Guide
Fourier components . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 493
13
Monte Carlo and sensitivity/worst-case analyses . . . . . . . . . . . 495
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Statistical analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of statistical analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Output control for statistical analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Model parameter values reports . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Monte Carlo history support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Waveform reports . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Collating functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Temperature considerations in statistical analyses . . . . . . . . . . . . . . . . . . . . . . . . .
Monte Carlo analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example: Monte Carlo analysis of a pressure sensor . . . . . . . . . . . . . . . . . . . . . . .
Monte Carlo Histograms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Worst-case analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of worst-case analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Worst-case analysis example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Tips and other useful information . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
495
496
496
497
497
498
503
504
505
506
512
521
528
528
531
535
14
Digital simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 539
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
What is digital simulation? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Steps for simulating digital circuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Concepts you need to understand . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
States . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Strengths . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining a digital stimulus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the DIGSTIMn part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Defining input signals using the Stimulus Editor . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the DIGCLOCK part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using STIM1, STIM4, STIM8 and STIM16 parts . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using the FILESTIMn parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
13
539
540
540
541
541
542
543
544
544
552
553
554
Product Version 10.5
PSpice User's Guide
Defining simulation time . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Adjusting simulation parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Selecting propagation delays . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Initializing flip-flops . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Starting the simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analyzing results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Adding digital signals to a plot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Adding buses to a waveform plot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Tracking timing violations and hazards . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
Mixed analog/digital simulation
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 577
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Interconnecting analog and digital parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Interface subcircuit selection by PSpice . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Level 1 interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Level 2 interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting the default A/D interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Specifying digital power supplies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Default power supply selection by PSpice A/D . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating custom digital power supplies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Interface generation and node names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
Digital worst-case timing analysis
14
577
578
579
580
581
582
583
583
585
589
. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 593
Digital worst-case timing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Digital worst-case analysis compared to analog worst-case analysis . . . . . . . . . . .
Starting digital worst-case timing analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Simulator representation of timing ambiguity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Propagation of timing ambiguity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Identification of timing hazards . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Convergence hazard . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Critical hazard . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Cumulative ambiguity hazard . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Reconvergence hazard . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
558
558
560
562
562
563
564
566
569
594
595
596
596
598
599
599
600
601
603
Product Version 10.5
PSpice User's Guide
Glitch suppression due to inertial delay . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 605
Methodology . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 606
Part four: Viewing results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 609
17
Analyzing waveforms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 611
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Overview of waveform analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Elements of a plot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Elements of a Probe window . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Managing multiple Probe windows . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up waveform analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up colors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing waveforms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up waveform display from Capture . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing waveforms while simulating . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using schematic page markers to add traces . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using display control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using plot window templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Limiting waveform data file size . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing large data files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using simulation data from multiple files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Saving simulation results in ASCII format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analog example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Mixed analog/digital tutorial . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
About digital states . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
About the oscillator circuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting up the design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Running the simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analyzing simulation results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
User interface features for waveform analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Zoom regions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Scrolling traces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Sizing digital plots . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
July 2005
15
611
612
613
614
615
617
617
622
622
623
626
630
633
646
650
658
663
665
669
669
670
670
671
671
674
674
676
676
Product Version 10.5
PSpice User's Guide
Modifying trace expressions and labels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Moving and copying trace names and expressions . . . . . . . . . . . . . . . . . . . . . . . . .
Copying and moving labels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Tabulating trace data values . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using cursors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Tracking digital simulation messages . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Message tracking from the message summary . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Message tracking from the waveform . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Trace expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Basic output variable form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Output variable form for device terminals . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analog trace expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Digital trace expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
678
679
680
681
682
687
687
689
689
690
692
700
703
18
Measurement expressions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 709
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Measurements overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Measurement strategy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Procedure for creating measurement expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Composing a measurement expression . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing the results of measurement evaluations . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing the results of measurement evaluations. . . . . . . . . . . . . . . . . . . . . . . . . . .
Measurement definitions included in PSpice . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
For power users . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating custom measurement definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Definition example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Measurement definition syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Syntax example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
709
710
711
712
712
712
713
714
717
718
721
721
722
725
734
19
Other output options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 737
Chapter overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 737
July 2005
16
Product Version 10.5
PSpice User's Guide
Viewing analog results in the PSpice window . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Writing additional results to the PSpice output file . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Generating plots of voltage and current values . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Generating tables of voltage and current values . . . . . . . . . . . . . . . . . . . . . . . . . . .
Generating tables of digital state changes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating test vector files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
738
739
739
741
742
743
A
Setting initial state . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 745
Appendix overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Save and load bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Save bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Load bias point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setpoints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Setting initial conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
745
746
746
747
748
750
B
Convergence and “time step too small errors” . . . . . . . . . . . . . . . 751
Appendix overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Newton-Raphson requirements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Is there a solution? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Are the equations continuous? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Is the initial approximation close enough? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Diagnostics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Bias Point (DC) Convergence . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
DC Sweep Convergence . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Transient Convergence . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
751
752
752
753
754
755
756
757
762
763
C
Importing Spice Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 771
Appendix Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 771
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 772
Importing text models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 772
July 2005
17
Product Version 10.5
PSpice User's Guide
Generating Part Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating New Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using symbols from an existing symbol library . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Model Import wizard . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Configuring new model library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Editing Model Editor created symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
773
773
775
778
779
781
D
PSpice SLPS Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 785
What is PSpice SLPS Interface? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 785
How to get PSpice SLPS Interface? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 786
Index. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 787
July 2005
18
Product Version 10.5
Before you begin
Welcome
OrCAD products offer a total solution for your core design
tasks: schematic- and VHDL-based design entry; FPGA and
CPLD design synthesis; digital, analog, and mixed-signal
simulation; and printed circuit board layout. What's more,
OrCAD 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 our total
solution design flow.
PSpice is a simulation program that models the behavior of a
circuit. PSpice simulates analog-only circuits, whereas
PSpice A/D simulates any mix of analog and digital 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
manufacturing the physical circuit board or IC.
PSpice User's Guide
19
Chapter
Before you begin
Product Version 10.5
How to use this guide
This guide is designed so you can quickly find the information
you need to use PSpice. To help you learn and use PSpice
efficiently, this manual is separated into the following sections:
■
Part 1 - Simulation primer
■
Part 2 - Design entry
■
Part 3 - Setting up and running analyses
■
Part 4 - Viewing results
Symbols and conventions
Our online documentation uses a few special symbols and
conventions.
Notation
Examples
Description
Ctrl+R
Press Ctrl+R
Means to hold down the Control key
while pressing R.
Alt, F, O
From the File menu, choose
Open (Alt, F, O).
Means that you have two options.
You can use the mouse to choose the
Open command from the File menu,
or you can press each of the keys in
parentheses in order: first Alt, then F,
then O.
Monospace font
In the Part Name text box, type
PARAM.
Text that you type is shown in
monospace font. In the example, you
type the characters P, A, R, A, and M.
UPPERCASE
In Capture, open
CLIPPERA.DSN.
Path and filenames are shown in
uppercase. In the example, you open
the design file named
CLIPPER.DSN.
Italics
In Capture, save
design_name.DSN.
Information that you are to provide is
shown in italics. In the example, you
save the design with a name of your
choice, but it must have an extension
of .DSN.
20
PSpice User's Guide
Product Version 10.5
Welcome
Related documentation
In addition to this guide, you can find technical product
information in the online help, online books, and our technical
web site, as well as in other books. The table below describes
the types of technical documentation provided with PSpice.
Note: The documentation you receive depends on the
software configuration you have purchased. Previous
editions of the PSpice User’s Guide focused only on
PSpice. The current PSpice User’s Guide supersedes
all other editions and covers PSpice A/D, PSpice A/D
Basics, and PSpice.
This documentation component . . . Provides this . . .
This guide—
PSpice User’s Guide
An online, searchable, comprehensive guide for
understanding and using the features available in
PSpice A/D, PSpice A/D Basics, and PSpice.
See Accessing online documentation on page 23
for information on how to access this online book.
PSpice Online help
Comprehensive information for understanding and
using the features available in PSpice A/D, PSpice
A/D Basics, and PSpice.
You can access help from the Help menu in PSpice
A/D, PSpice A/D Basics, or PSpice, by choosing the
Help button in a dialog box, or by pressing F1.
Topics include:
■
Explanations and instructions for common
tasks.
■
Descriptions of menu commands, dialog boxes,
tools on the toolbar and tool palettes, and the
status bar.
■
Error messages and glossary terms.
■
Reference information.
■
Product support information.
You can get context-sensitive help for a error
message by placing your cursor in the error
message line in the session log and pressing F1.
PSpice User's Guide
21
Chapter
Before you begin
Product Version 10.5
This documentation component . . . Provides this . . .
PSpice Advanced Analysis User’s
Guide
An online, searchable, comprehensive guide for
understanding and using the features available in
the PSpice Advanced Analysis add on program.
PSpice Advanced Analysis is an add-on option to
PSpice A/D and PSpice. PSpice Advanced
Analysis allows PSpice and PSpice A/D users to
optimize performance and improve quality of
designs before committing them to hardware.
Advanced Analysis’ four important capabilities:
sensitivity analysis, optimization, yield analysis
(Monte Carlo), and stress analysis (Smoke)
address design complexity as well as price,
performance, and quality requirements of circuit
design.
See Accessing online documentation on page 23
for information on how to access this online book.
PSpice Reference Guide
An online, searchable reference guide for PSpice
describing: detailed descriptions of the simulation
controls and analysis specifications, start-up option
definitions, and a list of device types in the analog
and digital model libraries. User interface
commands are provided to instruct you on each of
the screen commands.
See Accessing online documentation on page 23
for information on how to access this online book.
PSpice Library List
An online, searchable listing of all of the analog,
digital, and mixed-signal parts in the standard
model and part libraries that are shipped with
PSpice.
See Accessing online documentation on page 23
for information on how to access this online book.
22
PSpice User's Guide
Product Version 10.5
Welcome
This documentation component . . . Provides this . . .
PSpice Advanced Analysis Library
List
An online, searchable library list of components in
the Advanced Analysis libraries that are shipped
with PSpice.
The Advanced Analysis libraries contain
parameterized and standard components. The
parametrized components have tolerance,
distribution, optimizable and smoke parameters that
are required by the PSpice Advanced Analysis
tools.
See Accessing online documentation on page 23
for information on how to access this online book.
PSpice Quick Reference
Concise descriptions of the commands, shortcuts,
and tools available in PSpice.
See Accessing online documentation on page 23
for information on how to access this online book.
OrCAD Capture User’s Guide
Comprehensive information for understanding and
using the features available in the OrCAD Capture
schematic editor.
See Accessing online documentation on page 23
for information on how to access this online book.
Accessing online documentation
To access online documentation, you must open the Cadence
Documentation window.
1
Do one of the following:
❑
From the Windows Start menu, choose the
Release OrCAD 10.3 programs folder and then the
Online Documentation shortcut.
❑
From the Help menu in PSpice, choose Manuals.
The Cadence Documentation window appears.
2
PSpice User's Guide
Click the PSpice category to show the documents in the
category.
23
Chapter
Before you begin
Product Version 10.5
3
Double-click a document title to load that document into
your web browser.
What this user’s guide covers
PSpice is available in three versions:
❑
PSpice A/D
❑
PSpice A/D Basics
❑
PSpice
Note: An evaluation/academic version called PSpice A/D Lite
is also available.
This user’s guide is intended to provide a complete
understanding of how to use all of the features and
functionality provided by PSpice A/D. Because PSpice A/D
Basics and PSpice are each limited versions of the full PSpice
A/D product, their functionality is also described in this guide.
Note: For a summary of the differences between the versions
of PSpice, please see the sections below.
Wherever certain features or functions of PSpice A/D are
explained in this guide which are not available in one of the
other two versions, that limitation is noted.
If you are currently using PSpice A/D Basics or PSpice and
discover that you need the expanded capabilities offered by
PSpice A/D, you can easily upgrade without any loss of data
or conversion utilities. Any circuit file designed to simulate with
PSpice A/D Basics or PSpice will simulate with PSpice A/D.
PSpice A/D overview
PSpice A/D simulates analog-only, mixed analog/digital, and
digital-only circuits. PSpice A/D’s analog and digital
algorithms are built into the same program so that mixed
analog/digital circuits can be simulated with tightly-coupled
feedback loops between the analog and digital sections
without any performance degradation.
24
PSpice User's Guide
Product Version 10.5
Add-on options
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 A/D
for simulation. PSpice A/D formulates these into meaningful
graphical plots, which you can mark for display directly from
your schematic page using markers.
PSpice A/D Basics overview
PSpice A/D Basics provides the basic functionality needed for
analog and mixed-signal design without the advanced
features in the full PSpice A/D package.
PSpice overview
PSpice simulates analog circuits only, not mixed signal or
digital circuits. Otherwise, PSpice offers essentially the same
set of features and functionality as that provided by PSpice
A/D.
Note: For a more detailed list of the features and functionality
in each version of PSpice, see If you don’t have the
standard PSpice A/D package on page 26.
Add-on options
Besides PSpice, that are products that are available as add-on
options to PSpice or PSpice A/D and can be used to optimize
performance and reliability of their designs before committing
them to hardware.
These add-on options enable analog/mixed-signal circuit
designers to employ sophisticated design methodologies for
improving performance, time-to-market, and quality of design
while keeping the production costs in check.
PSpice Smoke Option
PSpice Smoke Option allows users to run smoke analysis on
their circuit designs.
PSpice User's Guide
25
Chapter
Before you begin
Product Version 10.5
PSpice Advanced Optimizer Option
PSpice Advanced Optimizer Option enables users to run
Optimizer, Monte Carlo, and Sensitivity analyses on their
circuit designs.
PSpice Advanced Analysis
The analyses covered in this bundle are Parametric Plotter,
Sensitivity, Optimizer, Smoke, and Monte Carlo.
Parametric Plotter provides the design exploration capabilities
to the designers. Using Parametric Plotter, you can perform
nested parametric sweep analysis on your circuit design.
Sensitivity Analysis shows graphically how much a change in
a design parameter affects your measurements. Optimizer
automates the iterative process of re-running simulations and
fine tuning your design. Smoke Analysis determines whether
components are operating within their safe operating limits.
Monte Carlo explores the parameter space bounded by
component tolerances and estimates the expected yield.
If you don’t have the standard PSpice A/D package
Comparison of the different versions of PSpice
The following table identifies which significant features are
included with PSpice A/D, PSpice A/D Basics, or PSpice.
Another version of PSpice A/D, called PSpice A/D Lite, is also
available. This product is intended for use by students, and is
provided for evaluation purposes as well. The limitations of
PSpice A/D Lite are listed after this table.
Note: For expert PSpice users, these are the PSpice circuit
file commands that are not available in the Basics
package:
26
❑
.STIMULUS
❑
.STIMLIB
PSpice User's Guide
Product Version 10.5
If you don’t have the standard PSpice A/D package
❑
.SAVEBIAS
❑
.LOADBIAS
For the most current information about the features and
functionality available in the different versions of PSpice,
contact PSpice Customer Support.
Comparison of PSpice product features
Feature
PSpice A/D PSpice A/D PSpice
(standard) Basics
Benefits of integration with OrCAD Capture
graphical design entry (schematic capture)
yes
yes
yes
simulation setup using dialog boxes
yes
yes
yes
cross-probing
yes
yes
yes
multi-window analysis of PSpice data sets
yes
yes
yes
marching waveforms in PSpice
yes
yes
yes
board layout package interfaces
yes
yes
yes
DC sweep, AC sweep, transient analysis
yes
yes
yes
noise, Fourier, temperature analysis
yes
yes
yes
parametric analysis
yes
no
yes
Monte Carlo, sensitivity/worst-case analysis
yes
no
yes
analog behavioral modeling (ABM)
yes
yes
yes
propagation delay modeling
yes
no
no
constraint checking (such as setup and hold
timing)
yes
no
no
digital worst-case timing
yes
no
no
charge storage on digital nets
yes
no
no
PSpice Stimulus Editor
yes
no
yes
PSpice Model Editor
yes
no1
yes
performance analysis (measurements)
yes
no
yes
Notable PSpice analysis and simulation features
PSpice User's Guide
27
Chapter
Before you begin
Product Version 10.5
Comparison of PSpice product features
Feature
PSpice A/D PSpice A/D PSpice
(standard) Basics
interactive simulation
yes
no
yes
preemptive simulation
yes
yes2
yes
save/load bias point
yes
no
yes
performance package
yes
no
yes
GaAsFETs: Curtice, Statz, TriQuint,
Parker-Skellern
all
Statz
all
MOSFETs: SPICE3 (1-3) with charge
conservation, BSIM1, BSIM3.1, EKV (version
2.6)
yes
yes
yes
IGBTs
yes
no
yes
JFETs, BJTs
yes
yes
yes
SCRs, thyristors
yes
no
yes
PWMs
yes
no
no
resistor, capacitor, and inductor .MODEL support yes
yes
yes
ideal, non-ideal lossy transmission lines
all
ideal
all
coupled inductors
yes
yes
yes
coupled transmission lines
yes
no
yes
nonlinear magnetics
yes
no
yes
voltage- and current-controlled switches
yes
yes
yes
analog model library
16,000+
12,000+
16,000+
digital primitives
all
most3
none
digital model library
1,600+
1,600+
0
advanced analysis library
4300+
0
4300+
PSpice Optimizer
yes
no
yes
Advanced Analysis
yes
no
yes
Notable PSpice devices and library models
Purchase options
28
PSpice User's Guide
Product Version 10.5
If you don’t have the standard PSpice A/D package
Comparison of PSpice product features
Feature
network licensing
PSpice A/D PSpice A/D PSpice
(standard) Basics
yes
no
yes
yes
no
yes
yes
yes5
yes
Other options
PSpice Device Equations Developer’s Kit
(DEDK)4
Miscellaneous specifications
unlimited circuit size
1.
2.
3.
4.
5.
Limited to text editing and diode device characterization.
Only allows one paused simulation in the queue.
PSpice A/D Basics does not include bidirectional transfer gates.
Available to qualified customers - contact PSpice Customer Support for qualification criteria.
Depends on system resources.
PSpice User's Guide
29
Chapter
Before you begin
Product Version 10.5
If you have PSpice A/D Lite
Limits of PSpice A/D Lite
PSpice A/D Lite has the following limitations:
■
circuit simulation limited to circuits with up to 64 nodes, 10
transistors, two operational amplifiers or 65 digital
primitive devices, and 10 transmission lines (ideal or
non-ideal) with not more than 4 pairwise coupled lines
■
device characterization using the PSpice Model Editor
limited to diodes
■
stimulus generation limited to sine waves (analog) and
clocks (digital)
■
sample library of approximately 39 analog and 134 digital
parts
■
displays only simulation data created using the demo
version of the simulator
■
PSpice Optimizer limited to one goal, one parameter and
one constraint
■
designs created in Capture can be saved if they have no
more than 30 part instances
Minimum hardware requirements for running PSpice:
30
■
Intel Pentium 300 MHz or equivalent processor
■
Windows XP Professional® (32-bit), Windows 2000 (with
Service Pack 2), and Windows NT 4.0 (with Service Pack
6a or higher).
■
64 MB RAM
■
256 MB swap space
■
150 MB of free hard disk space (in addition to Capture or
Capture CIS requirements)
■
A 256-color Windows display driver with 800 x 600
resolution (1024 x 768 recommended)
PSpice User's Guide
Product Version 10.5
PSpice User's Guide
If you don’t have the standard PSpice A/D package
■
CD-ROM drive
■
Mouse or similar pointing device
31
Chapter
32
Before you begin
Product Version 10.5
PSpice User's Guide
Part one: Simulation primer
Part one provides basic information about circuit simulation
including examples of common analyses.
PSpice User's Guide
■
Chapter 1, “Things you need to know,” provides an
overview of the circuit simulation process including what
PSpice does, descriptions of analysis types, and
descriptions of important files.
■
Chapter 2, “Simulation examples,” presents examples of
common analyses to introduce the methods and tools
you’ll need to enter, simulate, and analyze your design.
33
Chapter
34
Part one: Simulation primer
Product Version 10.5
PSpice User's Guide
Things you need to know
1
Chapter overview
This chapter introduces the purpose and function of the
PSpice A/D circuit simulator.
PSpice User's Guide
■
What is PSpice A/D? on page 36 describes PSpice A/D
capabilities.
■
Analyses you can run with PSpice A/D on page 40
introduces the different kinds of basic and advanced
analyses that PSpice A/D supports.
■
Using PSpice with other programs on page 46 presents
the high-level simulation design flow.
■
Files needed for simulation on page 47 describes the files
used to pass information between PSpice and other
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 53 describes the
files that contain simulation results.
■
New directory structure for analog projects on page 55
describes the new directory structure for analog projects.
35
Chapter 1
Things you need to know
Product Version 10.5
What is PSpice A/D?
PSpice A/D is a simulation program that models the behavior
of a circuit containing any mix of analog and digital devices.
Because the analog and digital simulation algorithms are built
into the same program, PSpice A/D simulates mixed-signal
circuits with no performance degradation because of tightly
coupled feedback loops between the analog and digital
sections.
Used with OrCAD Capture for design entry, you can think of
PSpice A/D 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 A/D 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.
Note: Parametric, Monte Carlo, and
sensitivity/worst-case analyses are not available in
PSpice A/D Basics.
■
Digital worst-case timing analysis to help you find timing
problems that occur with only certain combinations of
slow and fast signal transmissions.
Note: Digital worst-case timing analysis is not available
in PSpice and PSpice A/D Basics.
The range of models built into PSpice A/D include not only
those for resistors, inductors, capacitors, and bipolar
transistors, but also these:
■
36
transmission line models, including delay, reflection, loss,
dispersion, and crosstalk (no lossy in PSpice A/D Basics)
PSpice User's Guide
Product Version 10.5
Chapter overview
■
nonlinear magnetic core models, including saturation and
hysteresis (not in PSpice A/D Basics)
■
seven MOSFET models, including BSIM3 version 3.2 and
EKV version 2.6
■
five GaAsFET models, including Parker-Skellern and
TriQuint’s TOM2 model (only Statz in PSpice A/D Basics)
■
IGBTs (not in PSpice A/D Basics)
■
digital components with analog I/O models (not in
PSpice)
Use parts from PSpice’s extensive set of libraries
PSpice provides two types of libraries:
■
Standard PSpice libraries
■
PSpice Advanced Analysis libraries
Standard PSpice libraries
The standard PSpice libraries feature over 16,000 analog and
1,600 digital and mixed-signal models of devices
manufactured in North America, Japan, and Europe.
Use parts from standard PSpice libraries or PSpice Advanced
Analysis libraries if you want to analyze the part with PSpice.
The standard PSpice libraries are installed at the following
locations in the installation directory:
■
Capture symbols for standard PSpice libraries at
\tools\Capture\Library\PSpice\
■
Standard PSpice model libraries at
\tools\PSpice\Library\
The parts in the standard PSpice libraries are listed in the
online PSpice Library List. For information on finding parts
using the online PSpice Library List, see To find parts using
the online library lists on page 116. To find out more about
each model library, read the comments in the .LIB file header.
PSpice User's Guide
37
Chapter 1
Things you need to know
Product Version 10.5
PSpice Advanced Analysis libraries
The PSpice Advanced Analysis libraries contain over 4,300
analog parts. The Advanced Analysis libraries contain
parameterized and standard parts. The majority of the parts
are parameterized. The parametrized parts have tolerance,
distribution, optimizable and smoke parameters that are
required by the PSpice Advanced Analysis tools. Standard
parts in the Advanced Analysis libraries are similar to parts in
the standard PSpice libraries.
Note: The Advanced Analysis libraries are not available with
PSpice A/D Basics.
The parametrized parts are associated with template-based
PSpice models. An important advantage of using the
template-based PSpice models is that you can pass model
parameters as properties from Capture. For example, if a
template-based model is associated with a part, the model
parameters that you specify on an instance of the part in your
design will be passed to the model. There is no need to edit
the model itself to change a parameter value. This is unlike the
standard PSpice parts that are associated with device
characteristic curve-based PSpice models, where you need to
edit the model to change a simulation parameter. For more
information on template-based and device characteristic
curve-based PSpice models, see Chapter 4, “Creating and
editing models.”
Use parametrized parts from Advanced Analysis libraries if
you want to analyze the part with an Advanced Analysis tool.
Most of the analog parts in the standard PSpice libraries
contain smoke parameters. You can use these parts to
perform smoke analysis using the Smoke tool in PSpice
Advanced Analysis.
38
This Advanced
Analysis tool...
Uses these part parameters...
Sensitivity
Tolerance parameters
Optimizer
Optimizable parameters
Smoke
Smoke parameters
PSpice User's Guide
Product Version 10.5
Chapter overview
This Advanced
Analysis tool...
Uses these part parameters...
Monte Carlo
Tolerance parameters,
Distribution parameters
(default parameter value is Flat /
Uniform)
Note: You may use a mixture of standard and parameterized
parts in your design.
The Advanced Analysis libraries are installed at the following
locations in the installation directory:
■
Capture symbols for Advanced Analysis libraries at
\tools\Capture\Library\PSpice\AdvAnls\
■
PSpice Advanced Analysis model libraries at
\tools\PSpice\Library
The parts in the Advanced Analysis libraries are listed in the
PSpice Advanced Analysis Library List. For information
on finding parts using the online PSpice Advanced Analysis
Library List, see To find parts using the online library lists on
page 116. To find out more about each model library, read the
comments in the .LIB file header.
Vary device characteristics without creating new parts
PSpice A/D has numerous built-in models with parameters
that you can tweak for a given device. These include
independent temperature effects.
Model behavior
PSpice A/D supports analog and digital behavioral modeling,
so you can describe functional blocks of circuitry using
mathematical expressions and functions.
PSpice User's Guide
39
Chapter 1
Things you need to know
Product Version 10.5
Analyses you can run with PSpice A/D
■
See Chapter 2, “Simulation examples,” for introductory
examples showing how to run each type of analysis.
■
See Part three: Setting up and running analyses, for a more
detailed discussion of each type of analysis and how to
set it up.
Basic analyses
DC sweep & other DC calculations
These DC analyses evaluate circuit performance in response
to a direct current source. Table 1-1 summarizes what
PSpice A/D calculates for each DC analysis type.
Table 1-1 DC analysis types
For this DC
analysis...
PSpice A/D computes this...
DC sweep
Steady-state voltages, currents, and digital
states 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.
DC sensitivity
Sensitivity of a net or part voltage as a
function of bias point.
Small-signal
DC transfer
Small-signal DC gain, input resistance,
and output resistance as a function of bias
point.
AC sweep and noise
These AC analyses evaluate circuit performance in response
to a small-signal alternating current source. Table 1-2
40
PSpice User's Guide
Product Version 10.5
Chapter overview
summarizes what PSpice A/D calculates for each AC analysis
type.
Table 1-2 AC analysis types
For this AC
analysis...
PSpice A/D 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 also use Bode Plot
Template Windows in Probe to view this
information.
Noise
For each frequency specified in the AC
analysis:
■
Propagated noise contributions at an
output net from every noise generator
in the circuit.
■
RMS sum of the noise contributions at
the output.
■
Equivalent input noise.
Note: To run a noise analysis, you must also run an AC sweep
analysis.
PSpice User's Guide
41
Chapter 1
Things you need to know
Product Version 10.5
Transient and Fourier
These time-based analyses evaluate circuit performance in
response to time-varying sources. Table 1-3 summarizes what
PSpice A/D calculates for each time-based analysis type.
Table 1-3 Time-based analysis types
For this
time-based
analysis...
Transient
PSpice A/D computes this...
Voltages, currents, and digital states
tracked over time.
For digital devices, you can set the
propagation delays to minimum, typical,
and maximum. If you have enabled digital
worst-case timing analysis, then
PSpice A/D considers all possible
combinations of propagation delays within
the minimum and maximum range.
Note: Digital worst-case timing analysis is
not available in PSpice and
PSpice A/D Basics.
Fourier
DC and Fourier components of the
transient analysis results.
Note: To run a Fourier analysis, you must also run a transient
analysis.
42
PSpice User's Guide
Product Version 10.5
Chapter overview
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 A/D steps
a circuit value in a sequence that you specify and runs a
simulation for each value.
Note: Parametric and temperature analyses are not available
in PSpice A/D Basics.
Table 1-4 shows the circuit values that you can step for each
kind of analysis.
Table 1-4 Parametric and temperature analysis types
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 value.
Note: Monte Carlo and sensitivity/worst-case analyses are
not available in PSpice A/D Basics.
PSpice User's Guide
43
Chapter 1
Things you need to know
Product Version 10.5
Table 1-5 summarizes how PSpice runs each statistical
analysis type.
Table 1-5 Statistical analysis types
For this
statistical
analysis...
PSpice does this...
Monte Carlo
For each simulation, randomly varies all
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:
1. Computes component sensitivity to
changes in the device model parameters.
This means PSpice A/D nonrandomly
varies device model parameters for which
you have defined a tolerance, one at a
time for each device and runs a simulation
with each change.
2. Sets all model parameters for all devices
to their worst-case values (assumed to be
at one of the tolerance limits) and runs a
final simulation.
44
PSpice User's Guide
Product Version 10.5
Chapter overview
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.
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.
Perform post-simulation analysis of the results
This means you can plot additional information derived from
the waveforms. What you can plot 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.
Pinpoint design errors in digital circuits
When PSpice detects setup and hold violations, race
conditions, or timing hazards, a detailed message appears
along with corresponding waveforms. PSpice also helps you
locate the problem in your design.
PSpice User's Guide
45
Chapter 1
Things you need to know
Product Version 10.5
Using PSpice with other programs
Using OrCAD Capture to prepare for simulation
OrCAD 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.
OrCAD Capture is also the control point for running other
programs used in the simulation design flow.
What is the PSpice Stimulus Editor?
The Stimulus Editor is a graphical input waveform editor 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:
46
■
analog stimuli with sine wave, pulse, piecewise linear,
exponential pulse, single-frequency FM shapes, and
■
digital stimuli that range from simple clocks to complex
pulse patterns and bus sequences.
PSpice User's Guide
Product Version 10.5
Files needed for simulation
The Stimulus Editor lets you draw analog piecewise linear and
all digital stimuli by clicking at the points along the timeline that
correspond to the input values that you want at transitions.
Note: The Stimulus Editor is not available in
PSpice A/D Basics.
What is the PSpice Model Editor?
The PSpice Model Editor is a model extractor that generates
model definitions for PSpice A/D to use during simulation.
All the PSpice 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 PSpice
Model Editor automatically creates a part for the model so you
can use the modeled part in your design immediately.
Note: In PSpice A/D Basics, the PSpice Model Editor is
available but is limited to text editing and diode device
characterization.
Files needed for simulation
To simulate your design, PSpice needs to know about:
PSpice User's Guide
■
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
47
Chapter 1
Things you need to know
■
Product Version 10.5
the stimulus definitions to test with.
This information is provided in various data files. Some of
these are generated by OrCAD Capture, others come from
libraries (which can also be generated by other programs like
the PSpice Stimulus Editor and the PSpice Model Editor), and
still others are user-defined.
Files that OrCAD Capture generates
When you begin the simulation process, OrCAD 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
The netlist file contains a list of device names, values, and how
they are connected with other devices.
The name that OrCAD Capture generates for this file is:
■
ROOT_SCHEMATIC_NAME.NET, if you have updated
your project to the new project format. For more
information on the new format for analog projects, see
Conversion of old analog projects to new project
format in the OrCAD Capture Online Help and New
directory structure for analog projects on page 55.
In the new project format, the netlist file is located in the
directory:
\<project_name>-PSpiceFiles\<schematic_name>\
■
DESIGN_NAME-ROOT_SCHEMATIC_NAME.NET, if you
did not update your project to the new project format. In
the old format for analog projects, the netlist file is located
in the project directory.
Refer to the online PSpice Reference Guide for the syntax
of the statements in the netlist file.
48
PSpice User's Guide
Product Version 10.5
Files needed for simulation
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 OrCAD Capture generates for this file is:
■
PROFILE_NAME.CIR, if you updated your project to the
new project format. For more information on the new
format for analog projects, see Conversion of old
analog projects to new project format in the OrCAD
Capture Online Help and New directory structure for
analog projects on page 55.
In the new project format, the circuit file is located in the
directory:
\<project_name>-PSpiceFiles\<schematic_name>\<prof
ile_name>\
■
DESIGN_NAME-ROOT_SCHEMATIC_NAME-PROFILE_NAM
E.SIM.CIR, if you did not update your project to the new
project format. In the old format for analog projects, the
circuit file is located in the project directory.
Refer to the online PSpice Reference Guide for the syntax
of the statements in the circuit file.
PSpice User's Guide
49
Chapter 1
Things you need to know
Product Version 10.5
Other files that you can configure for simulation
PSpice
Stimulus Editor
global
model
libraries
PSpice
Model Editor
model
definitions
input
waveforms
stimulus file
simulation
primitives
local
model
libraries
custom
include file
PSpice A/D
Figure 1-1 User-configurable data files that PSpice A/D
reads.
Before starting simulation, PSpice needs to read other files
that contain simulation information for your circuit. These are
model files, and if required, stimulus files and include files.
You can create these files using PSpice programs like the
PSpice Stimulus Editor and the PSpice 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 PSpice Model Editor (or another text editor like
Notepad) to enter the data manually.
The circuit file (.CIR) that OrCAD Capture generates contains
references to the other user-configurable files that PSpice
needs to read.
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.
50
PSpice User's Guide
Product Version 10.5
Files needed for simulation
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
■
subcircuit netlist, which describes the structure and
function of the part by interconnecting other parts and
primitives.
A subcircuit, sometimes called a macromodel, is
analogous to a procedure call in a software programming
language.
The most commonly used models are available in the PSpice
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 PSpice Model
Editor (or another text editor like Notepad), or
■
automatically using the PSpice Model Editor.
See What is the PSpice Model Editor? on page 47 for a
description.
Stimulus file
A stimulus file contains time-based definitions for analog or
digital input waveforms. You can create a stimulus file either:
■
manually using a standard text editor such as Notepad to
create the definition (a typical file extension is .STM), or
■
automatically using the Stimulus Editor (which generates
a .STL file extension).
See What is the PSpice Stimulus Editor? on page 46 for a
description.
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 properties.
PSpice User's Guide
51
Chapter 1
Things you need to know
Product Version 10.5
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 PSpice output file on
page 53).
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.
You can create an include file using any text editor, such as
Notepad. Typically, include file names have an .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.
The files that PSpice searches depend on how you configure
your model libraries and other files. Much of the configuration
is set up for you automatically, however, you can do the
following yourself:
■
Add and delete files from the configuration.
■
Change the scope of a file: that is, whether the file applies
to one profile only, one design only (local) or to any design
(global).
■
Change the search order.
Libraries are configured by editing the simulation profile. From
the PSpice menu in OrCAD Capture, choose Edit Simulation
Profile, click the Configuration Files tab in the Simulation
Settings dialog box, then click Library in the Category field. To
find out more, refer to the OrCAD Capture User’s Guide.
52
PSpice User's Guide
Product Version 10.5
Files that PSpice generates
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 results to two files—the
data file and the PSpice output file.
Waveform data file
The data file contains simulation results that can be displayed
graphically. PSpice reads this file automatically 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.
For a description of how to display simulation results, see Part
four: Viewing results. For a description of the waveform
analyzer program, see What is waveform analysis? on
page 45.
After PSpice has read the data file and displays the initial set
of results, you can add more waveforms and perform
post-simulation analysis of the data. There are two ways to
add waveforms to the display:
■
From within PSpice, by specifying trace expressions.
■
From within OrCAD Capture, by cross-probing.
PSpice output file
The PSpice output file is an ASCII text file that contains:
PSpice User's Guide
■
the netlist representation of the circuit,
■
the PSpice command syntax for simulation commands
and options (like the enabled analyses),
■
simulation results, and
■
warning and error messages for problems encountered
during read-in or simulation.
53
Chapter 1
Things you need to know
Product Version 10.5
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, available in SPECIAL.OLB) that you place and
connect to nets in your design.
Example: Each instance of a VPRINT1 symbol placed in
your schematic causes PSpice to generate a table of
voltage values for the connecting net, and to write the
table to the PSpice output file.
54
PSpice User's Guide
Product Version 10.5
Files that PSpice generates
New directory structure for analog projects
The files related to analog projects created using
OrCAD Capture version 9.2.3 or older versions were
maintained in a single directory.
Figure 1-2 Directory structure for RF_AMP analog
project created using Capture 9.2.3 or older versions
In the above figure, the rf_amp project has a design named
rf_amp.dsn. The rf_amp design has a schematic named
SCHEMATIC1 and SCHEMATIC1 has two profiles,
rf_amp-schematic1-ac.sim and
rf_amp-schematic1-tran.sim. The long file names
make it difficult to identify files associated with the design,
schematic or profile, and delete them if they are no longer
required. For example, the .sim (simulation profile) files have
the name,
PSpice User's Guide
55
Chapter 1
Things you need to know
Product Version 10.5
<DesignName>-<SchematicName>-<ProfileName>.SIM
Capture 10.0 introduces a new directory structure for analog
projects in which the design level, schematic level and
simulation profile level PSpice files are organized in their
respective directories. This makes it easier to manage the files
for the project.
Note: If you open an analog project that was created using
Capture version 9.2.3 or older versions in Capture
10.0, you will be prompted to convert the project to the
Capture 10.0 format. For more information, see
Conversion of old analog projects to new project
format in the OrCAD Capture Online Help.
56
PSpice User's Guide
Product Version 10.5
Files that PSpice generates
Project
directory
Directory for
design level
PSpice files
Directory for
schematic level
PSpice files
Directory for
profile level
PSpice files
Figure 1-3 New directory structure of RF_AMP
analog project
In the new directory structure all the PSpice related files for
the rf_amp project are maintained in a directory named
rf_amp-PSpiceFiles.
■
PSpice User's Guide
The PSpice files related to the design are maintained in
the rf_amp-PSpiceFiles directory. For more
57
Chapter 1
Things you need to know
Product Version 10.5
information, see How are files configured at the design
level maintained in the new directory structure for analog
projects? on page 58.
■
The PSpice files related to the schematic named
SCHEMATIC1 are maintained in a sub-directory named
SCHEMATIC1 under the rf_amp-PSpiceFiles
directory.
■
The PSpice files related to the AC and Tran simulation
profiles are maintained in the AC and Tran
sub-directories under the SCHEMATIC1 directory. For
more information, see How are files configured at the
profile level maintained in the new directory structure for
analog projects? on page 60.
How are files configured at the design level maintained in the new directory
structure for analog projects?
The model libraries, stimulus files and include files configured
at the design level are stored in the
<projectname>-PSpiceFiles directory. For example, in
the New directory structure of RF_AMP analog project figure
on page 57, the model libraries, stimulus files and include files
configured at the design level are stored in the
rf_amp-PSpiceFiles directory. The rf_amp.stl
stimulus file in the rf_amp-PSpiceFiles directory is an
example of a PSpice file related to the design.
You can view the paths to the model libraries, stimulus files
and include files configured at the design level in the Capture
Project Manager window.
Note the following:
■
58
If you select the Retain Old Project check box when you
convert an analog project that was created using Capture
version 9.2.3 or older versions to the new project format,
only the files configured at the design level that have the
same name as the design are copied over to the
<projectname>-PSpiceFiles directory in the
location you specified for creating the project in the new
format.
PSpice User's Guide
Product Version 10.5
Files that PSpice generates
The files configured at the design level that do not have
the same name as the design are not copied over to the
<projectname>-PSpiceFiles directory because
they are custom files. Instead, these files are read from
their original location. You can view the path to the
custom files configured at the design level in the
Configuration Files tab of the Simulation Settings dialog
box and in the Capture Project Manager window.
For example, suppose that your design name is rf_amp,
and you have configured the following files at the design
level:
❑
rf_amp.inc
❑
decoder.lib
❑
rf_amp.lib
❑
rf_amp.prp
❑
rf_amp.stl
If you select the Retain Old Project check box when you
convert the analog project to the new format, only the
following files are copied over to the
rf_amp-PSpiceFiles directory in the location you
specified for creating the project in the new format.
❑
rf_amp.inc
❑
rf_amp.lib
❑
rf_amp.prp
❑
rf_amp.stl
The decoder.lib file is read from the old project
location. You can view the path to the decoder.lib file
in the Configuration Files tab of the Simulation Settings
dialog box and in the Capture Project Manager window.
For more information on converting analog projects from
the old format to the new format, see Conversion of old
analog projects to new project format in the OrCAD
Capture Online Help.
PSpice User's Guide
59
Chapter 1
Things you need to know
■
Product Version 10.5
When you create a new simulation profile by importing
the settings from another simulation profile that exists in
another project, only the simulation settings are inherited
from the source simulation profile. The files configured at
the design level for the source simulation profile are not
copied over to the <projectname>-PSpiceFiles
directory of the project in which you are creating the new
simulation profile.
How are files configured at the profile level maintained in the new
directory structure for analog projects?
The model libraries, stimulus files and include files configured
at the profile level are stored in a directory that has the same
name as the profile. For example, in Figure 1-4, the PSpice
files related to the Tran simulation profile are maintained in the
Tran sub-directory under the SCHEMATIC1 directory.
60
PSpice User's Guide
Product Version 10.5
Files that PSpice generates
Figure 1-4 Directory structure of RF_AMP analog project
with files configured for the Tran profile
PSpice User's Guide
61
Chapter 1
Things you need to know
Product Version 10.5
An include file named <profilename>_profile.inc is
created in the directory for the simulation profile. This file
contains information on the model libraries, stimulus files and
include files configured for that profile. For example, in
Figure 1-4, the Tran profile directory contains a
Tran_profile.inc include file that includes information on
the decoder.lib model library, decoder.stl stimulus file
and the Tran.inc include files configured for the Tran profile.
You must not delete the <profilename>_profile.inc file
in the directory for a simulation profile.
Note: When you create a new simulation profile by importing
the settings from another simulation profile that exists
in the same project or in another project, the files
configured at the profile level for the source simulation
profile are copied to the directory for the new simulation
profile. The files configured at the design level for the
source simulation profile are not copied over to the
<projectname>-PSpiceFiles directory of the
project in which you are creating the new simulation
profile.
What happens when I convert an analog project that uses a design from
another project or from another location?
If you convert an analog project (created using Capture 9.2.3
or older versions) that uses a design from another project or
from another location, to the new project format, the design file
and all the contents of the design are copied to the current
project and maintained in the new directory structure for
analog projects.
What should I do if the schematic for a converted analog project uses
FILESTIMn parts from the SOURCE library?
If you have specified only the name of the stimulus file as the
value of the FILENAME property on a FILESTIMn part, you
must specify the path to the stimulus file in the value for the
FILENAME property on the FILESTIMn part.
62
PSpice User's Guide
Simulation examples
2
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:
PSpice User's Guide
■
Example circuit creation on page 64
■
Performing a bias point analysis on page 73
■
DC sweep analysis on page 76
■
Transient analysis on page 83
■
AC sweep analysis on page 88
■
Parametric analysis on page 93
■
Performance analysis on page 101
63
Chapter 2
Simulation examples
Product Version 10.5
Example circuit creation
This section describes how to use OrCAD Capture to create
the simple diode clipper circuit shown in Figure 2-1.
Figure 2-1 Diode clipper circuit.
To create a new PSpice project
64
1
From the Windows Start menu, choose Release OrCAD
10.0 from the Programs 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 or Mixed-Signal Circuit Wizard.
4
In the Name text box, enter the name of the project
(CLIPPER).
5
Use the Browse button to select the location for the
project files, then click OK.
6
In the Create PSpice Project dialog box, select Create a
blank project.
7
Click OK.
PSpice User's Guide
Product Version 10.5
Chapter overview
No special libraries need to be configured at this 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.
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.
Note: There are two sets of library files supplied with
Capture and PSpice. The standard schematic part
libraries are found in the directory
\TOOLS\CAPTURE\LIBRARY. The part libraries that are
designed for simulation with PSpice are found in the
sub-directory \TOOLS\CAPTURE\LIBRARY\PSPICE. In
order to have access to specific parts, you must first
configure the library in Capture using the Add Library
function.
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 2-1) 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
PSpice User's Guide
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:
65
Chapter 2
Simulation examples
Product Version 10.5
a. Click the Add Library button.
b. Select DIODE.OLB (from the PSpice library) and
click Open.
Important
If you are working with the demo version of Capture,
add EVAL.OLB instead of DIODE.OLB.
3
In the Part text box, type D1N39 to display a list of diodes.
When placing parts:
4
❑
Leave space to connect the parts with wires.
❑
You will change part names and values that do not
match those shown in Figure 2-1 later in this section.
Select D1N3940 from the Part List and click OK.
Important
If you are working with the demo version of Capture,
select D1N914 from the Part List.
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.
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
66
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:
PSpice User's Guide
Product Version 10.5
Chapter overview
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, according to Figure 2-1 on
page 64. 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 2-1 on page 64.
Note: To rotate the part so the arrows are pointing in the
correct direction, place the part, select it, then press R
one or more times to rotate the part to the desired
orientation.
To place the zero ground part
1
PSpice User's Guide
To place the ground parts (0), click the GND
button
on the tool palette.
67
Chapter 2
Simulation examples
Product Version 10.5
2
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.
3
Place the 0 ground part from SOURCE.OLB as shown in
Figure 2-1 on page 64.
Important
You must use the 0 (zero) ground part from the
SOURCE.OLB part library. You can use any other
ground part only if you change its name to 0 (zero).
To connect the parts
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.
To stop wiring, right-click and choose End Wire. The
pointer changes to the default arrow.
Clicking on any valid connection point ends a wire. A valid
connection point is shown as a box (see Figure 2-2).
Figure 2-2 Connection points.
If you make a mistake when placing or connecting
components:
From the Edit menu, choose Undo, or click
4
68
.
Connect the other end of R1 to the output capacitor.
PSpice User's Guide
Product Version 10.5
Chapter overview
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 2-1 on page 64.
To assign names (labels) to the nets
1
From the Place menu, choose Net Alias to display the
Place Net Alias dialog box.
2
In the Name text box, type Mid.
3
Click OK.
4
Place the net alias on any segment of the wire that
connects R1, R2, R3, the diodes, and the capacitor. The
lower left corner of the net alias must touch the wire.
5
Right-click and choose End Mode to quit the Net Alias
function.
Tip
It is recommended that special characters should not
be used for naming nets, nodes, projects, or libraries.
While naming nets, characters such as ? (question
mark), @ (at symbol), ~ (telda), #(hash), &
(ampersand), %(percent sign), and “ (quotation
marks) should not be used. These might cause the
netlister to fail. Other special characters such as
! (exclamation mark), ( )(paranthesis), < (smaller
than), = (equal), > (greater than), [ ](square
parenthesis), and * (asterix) are also considered as
illegal for naming nets.
PSpice User's Guide
69
Chapter 2
Simulation examples
Product Version 10.5
To assign names (labels) to the off-page connectors
Label the off-page connectors as shown in Figure 2-1 on
page 64.
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
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 2-1 on page 64.
Tip
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:
a. Select all of the parts to be modified by pressing Ctrl
and clicking each part.
b. 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.
70
PSpice User's Guide
Product Version 10.5
Chapter overview
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 5V.
3
Click OK.
4
Continue changing the Part Value properties of the parts
until all the parts are defined as in Figure 2-1 on page 64.
Your schematic page should now have the same parts,
wiring, labels, and properties as Figure 2-1 on page 64.
Using European notation
You can use the European notation, such as 2K2, to assign
values to resistors, capacitors, and inductors. Assigning
values in this format reduces the possibility of errors while
reading component values from screen or from a print out of
the schematic. The table below lists the alphabets that can be
used in the 2K2 notation.
PSpice User's Guide
Alphabet used..
Stands for..
F(f)
femto
P(p)
pico
N(n)
nano
U(u)
micro
M(m)
milli
K(k)
kilo
MEG(meg)
mega
G(g)
giga
T(t)
tera
71
Chapter 2
Simulation examples
Product Version 10.5
Some examples and their explanations are listed in the table
below.
Notations
Equivalent to...
2M2
2.2 M
2MEG2
2.2 MEG
4L5
inductor of 4.5 henry
2K2
2.2K
12C2
capacitor of 12.2 farads
5R4
resistor of 5.4 ohms
2p2
2.2 p (2.2*10-12)
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 set up your
design for simulation, and how to avoid common problems,
see Chapter 3, “Preparing a design for simulation.”
Running PSpice
When you perform a simulation, PSpice generates an output
file (*.OUT).
72
PSpice User's Guide
Product Version 10.5
Running PSpice
While PSpice is running, the progress of the simulation
appears and is updated in the PSpice simulation output
window (see Figure 2-3).
Figure 2-3 PSpice simulation output window.
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 Chapter 8, “Setting up analyses and starting
simulation.”
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.
3
In the Name text box, type Bias.
4
From the Inherit From list, select None, then click Create.
The Simulation Settings dialog box appears.
The root schematic listed is the schematic page
associated with the simulation profile you are creating.
PSpice User's Guide
5
From the Analysis type list, select Bias Point.
6
Click OK to close the Simulation Settings dialog box.
73
Chapter 2
Simulation examples
Product Version 10.5
To simulate the circuit from within Capture
1
From the PSpice menu, choose Run.
PSpice simulates the circuit and calculates the bias point
information.
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.
74
PSpice User's Guide
Product Version 10.5
Running PSpice
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 anomalies while performing the
calculation, PSpice writes error or warning messages to the
output file.
To view the simulation output file
1
In PSpice, from the View menu, choose Output File.
Figure 2-4 shows the results of the bias point calculation
as written in the simulation output file.
Figure 2-4 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 measured 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.
PSpice User's Guide
75
Chapter 2
Simulation examples
Product Version 10.5
Finding out more about bias point calculations
To find out more about
this...
See this...
Bias point calculations
Bias point on page 429
DC sweep analysis
You can visually verify the DC response of the clipper 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.
2
In the Name text box, type DC Sweep.
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 2-5.
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
76
PSpice User's Guide
Product Version 10.5
DC sweep analysis
variable and Sweep type.
Figure 2-5 DC sweep analysis settings.
PSpice User's Guide
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.
77
Chapter 2
Simulation examples
Product Version 10.5
Displaying DC analysis results
Probe windows can appear during or after the simulation is
finished.
Figure 2-7 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
78
From Capture’s PSpice menu, point to Markers and
choose Voltage Level.
PSpice User's Guide
Product Version 10.5
DC sweep analysis
2
Click to place a marker on net Out, as shown in Figure
2-8.
Figure 2-8 Clipper circuit with voltage marker on n
Out.
3
Right-click and choose End Mode to stop placing
markers.
4
From the File menu, choose Save.
5
Switch to PSpice. The V(Out) waveform trace appears, as
shown in Figure 2-9.
Figure 2-9 Voltage at In, Mid, and Out.
PSpice User's Guide
79
Chapter 2
Simulation examples
Product Version 10.5
To place cursors on V(In) and V(Mid)
This example uses the cursors feature to view the numeric
values for two traces and the difference between them by
placing a cursor on each trace.
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 crosshairs for the second
cursor.
Table 2-1 Association of cursors with mouse
buttons.
cursor 1
left mouse button
cursor 2
right mouse button
In the trace legend, the part for V(In) is outlined in the
crosshair pattern for each cursor, resulting in a dashed
line as shown in Figure 2-10.
Figure 2-10 Trace legend with cursors activated.
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,
80
PSpice User's Guide
Product Version 10.5
DC sweep analysis
and the current X and Y values for the first cursor
appear in the cursor window.
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 Right arrow key and Left
arrow key for tighter control.
Note: Your ability to get as close to 4.0 as possible
depends on screen resolution and window size.
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 2-11.
Figure 2-11 Trace legend with V(Mid)
symbol outlined.
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-tune 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 Shift+Right
arrow key and Shift+Left arrow key for tighter
control.
PSpice User's Guide
81
Chapter 2
Simulation examples
Product Version 10.5
Figure 2-12 shows the Probe window with both cursors
placed.
Figure 2-12 Voltage difference at V(In) = 4 volts.
There are also ways to display the difference between two
voltages as a trace:
■
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.
To delete all of the traces
1
From the Trace menu, choose Delete All Traces.
Note: You can also delete an individual trace by selecting
its name in the trace legend and then pressing Delete.
Example: To delete the V(In) trace, click the text, V(In),
located under the plot’s x-axis, and then press Delete.
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.
82
PSpice User's Guide
Product Version 10.5
Transient analysis
Finding out more about DC sweep analysis
To find out more about
this...
See this...
DC sweep analysis
DC Sweep on page 420
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 2-13.
Figure 2-13 Diode clipper circuit with a voltage stimulus.
To add a time-domain voltage stimulus
PSpice User's Guide
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.
83
Chapter 2
Simulation examples
Product Version 10.5
4
Scroll down (or from the View menu, point to Zoom, then
choose Out).
5
Place a VSTIM part (from the PSpice library
SOURCSTM.OLB) as shown in Figure 2-13.
6
From the Edit menu, choose Paste.
7
Place the ground part under the VSTIM part as shown in
Figure 2-13.
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
Note: The Stimulus Editor is not available in
PSpice A/D Basics. If you are using
PSpice A/D Basics, see If you do not have the
Stimulus Editor on page 85.
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 SINE.
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
84
Click Apply to view the waveform.
PSpice User's Guide
Product Version 10.5
Transient analysis
The Stimulus Editor window should look like Figure 2-14.
Figure 2-14 Stimulus Editor window.
7
Click OK.
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.
If you do not have the Stimulus Editor
1
Place a VSIN part instead of VSTIM and double-click it.
2
In the Edit Part dialog box, click User Properties.
3
Set values for the VOFF, VAMPL, and FREQ properties
as defined in step 5. When finished, click OK.
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
PSpice User's Guide
In the Name text box, type Transient.
85
Chapter 2
Simulation examples
Product Version 10.5
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 2-15.
Figure 2-15 Transient
analysis simulation
settings.
TSTOP = 2ms
Start saving data after = 20ns
6
Click OK to close the Simulation Settings dialog box.
7
From the PSpice menu, choose Run to perform the
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.
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 simulation output file (*.OUT).
To display the input sine wave and clipped wave at V(Out)
86
1
From PSpice’s Trace menu, choose Add Trace.
2
In the trace list, select V(In) and V(Out) by clicking them.
PSpice User's Guide
Product Version 10.5
Transient analysis
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.
Figure 2-16 Sinusoidal input and clipped output
waveforms.
The waveforms illustrate the clipping of the input signal.
Finding out more about transient analysis
To find out more about
this...
See this...
transient analysis for analog
and mixed-signal designs1
Chapter 12, “Transient
analysis”
transient analysis for digital
designs1
Chapter 14, “Digital
simulation”
1. Includes how to set up time-based stimuli using the Stimulus
Editor.
PSpice User's Guide
87
Chapter 2
Simulation examples
Product Version 10.5
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 2-17) and by setting up AC sweep parameters.
Figure 2-17 Clipper circuit with AC stimulus.
To change Vin to include the AC stimulus signal
88
1
In Capture, open CLIPPER.OPJ.
2
Select the DC voltage source, Vin, and press D to remove
the part from the schematic page.
3
From the Place menu, choose Part.
4
In the Part text box, type VAC (from the PSpice library
SOURCE.OLB) and click OK.
PSpice User's Guide
Product Version 10.5
Transient analysis
5
Place the AC voltage source on the schematic page, as
shown in Figure 2-17.
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.
Note: PSpice simulation is not case-sensitive, so both M
and m can be used as “milli,” and MEG, Meg, and meg
can all be used for “mega.” However, waveform analysis
treats M and m as mega and milli, respectively.
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 AC Sweep/Noise and
enter the settings shown in Figure 2-18.
Figure 2-18 AC sweep and noise analysis
simulation settings.
PSpice User's Guide
89
Chapter 2
Simulation examples
Product Version 10.5
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
1
From Capture’s PSpice menu, point to Markers, point to
Advanced, then choose db Magnitude of Voltage.
Note: You must first define a simulation profile for the AC
Sweep/Noise analysis in order to use advanced markers.
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 magnitude (20log10) of the voltage at
the marked nets, Out and Mid, in a Probe window as shown in
Figure 2-19 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
90
PSpice User's Guide
Product Version 10.5
Transient analysis
to 1V, the output voltage is the same as the gain (or
attenuation) of the circuit.
Figure 2-19 dB magnitude curves for “gain” at Mid and
Out.
To display a Bode plot of the output voltage, including
phase
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.
Note: Depending upon where the Vphase marker was
placed, the trace name may be different, such as
VP(Cout:2), VP(R4:1).
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.
For more information on Probe windows and trace
expressions, see Chapter 17, “Analyzing waveforms.”
PSpice User's Guide
5
Click the trace name VP(Out) to select the trace.
6
From the Edit menu, choose Cut.
91
Chapter 2
Simulation examples
Product Version 10.5
7
From the Plot menu, choose Add Y Axis.
8
From the Edit menu, choose Paste.
The Bode plot appears, as shown in Figure 2-20.
Figure 2-20 Bode plot of clipper’s frequency response.
Finding out more about AC sweep and noise analysis
92
To find out more about
this...
See this...
AC sweep analysis
AC sweep analysis on
page 438
noise analysis based on an
AC sweep analysis
Noise analysis on page 448
PSpice User's Guide
Product Version 10.5
Transient analysis
Parametric analysis
Note: Parametric analysis is not included in PSpice A/D
Basics.
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 2-21 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 A/D.
PSpice User's Guide
93
Chapter 2
Simulation examples
Product Version 10.5
Setting up and running the parametric analysis
To change the value of R1 to the expression {Rval}
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 {Rval}.
PSpice interprets text 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.
4
Click OK.
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 PARAM (from the PSpice 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.
For more information about using the Parts spreadsheet,
see the OrCAD Capture User’s Guide.
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.
94
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.
PSpice User's Guide
Product Version 10.5
Transient analysis
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 Delete to remove the
marker from the schematic page.
Note: This example is only interested in the magnitude of
the response.
12 From the File menu, choose Save to save the design.
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.
2
In the Name text box, type Parametric.
3
From the Inherit From list, select AC Sweep, then click
Create.
The Simulation Settings dialog box appears.
The root schematic listed is the schematic page
associated with the simulation profile you are creating.
4
PSpice User's Guide
Click the Analysis tab.
95
Chapter 2
Simulation examples
Product Version 10.5
5
Under Options, select Parametric Sweep and enter the
settings as shown below.
Figure 2-22 Parametric simulation settings.
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 value of R1 as it logarithmically increases from 100Ω
to 10 kΩ in 20 steps, resulting in a total of 21 runs.
96
6
Click OK.
7
From the PSpice menu, choose Run to start the analysis.
PSpice User's Guide
Product Version 10.5
Transient 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 select individual
runs, click each one separately.
To display all 21 traces
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 2-23.
Figure 2-23 Small signal response as R1 is varied
from 100Ω to 10 kΩ.
To see more information about the section that produced
a specific trace, double-click the corresponding symbol in
the legend below the x-axis.
2
Click the trace name to select it, then press Delete to
remove the traces shown.
You can also remove the traces by removing the VDB
marker from your schematic page in Capture.
PSpice User's Guide
97
Chapter 2
Simulation examples
Product Version 10.5
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:
Vdb(Out)@1 Vdb(Out)@21
Tip
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.
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 Trace 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.
c. From the Trace menu, point to Cursor and choose
Max.
98
PSpice User's Guide
Product Version 10.5
Transient analysis
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)
The search command tells PSpice to search for the
point on the trace where the x-axis value is 100.
f. Select 2 as the Cursor to Move option.
g. Click OK.
Figure 2-24 shows the Probe window with cursors placed.
Figure 2-24 Small signal frequency response
at 100 and 10 kΩ input resistance.
Note that the Y value for cursor 2 in the cursor box is
about 17.87. This indicates that when R1 is set to 10 kΩ,
the small signal attenuation of the circuit at 100Hz is
17.87dB greater than when R1 is 100Ω.
PSpice User's Guide
6
From the Trace menu, point to Cursor and choose Display
to turn off the display of the cursors.
7
Delete the trace.
99
Chapter 2
Simulation examples
Product Version 10.5
Finding out more about parametric analysis
100
To find out more about
this...
See this...
parametric analysis
Parametric analysis on
page 458
using global parameters
Using global parameters and
expressions for values on
page 121
PSpice User's Guide
Product Version 10.5
Transient analysis
Performance analysis
Note: Performance analysis is not available in
PSpice A/D Basics.
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.
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.
Note: The Performance Analysis menu item is only
available if an analysis data file is available. In this case,
the data from the parametric analysis of the previous
example should still be open.
3
Click the Wizard button.
At each step, the wizard provides information and
guidelines.
4
PSpice User's Guide
Click the Next> button.
101
Chapter 2
Simulation examples
Product Version 10.5
5
In the Choose a Goal Function list, click Bandwidth, then
click the Next> button.
6
Click in the Name of Trace to search text box and type
V(Out).
7
Click in the db level down for bandwidth calc text box and
type 3.
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.
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:
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
Measurements list, and then click the Max(1) goal
function.
The Trace list includes measurements expressions only
in performance analysis mode when the x-axis variable is
the swept parameter.
102
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 User's Guide
Product Version 10.5
Transient analysis
PSpice displays gain on the second y-axis vs. Rval.
Figure 2-25 shows the final performance analysis plot of 3dB
bandwidth and gain in dB vs. the swept input resistance value.
Figure 2-25 Performance analysis plots of bandwidth and
gain vs. Rval.
Finding out more about performance analysis
To find out more about
this...
See this...
how to use performance
analysis
RLC filter example on
page 459
Example: Monte Carlo
analysis of a pressure sensor
on page 512
how to use search
commands and create
measurement expressions
PSpice User's Guide
Chapter 18, “Measurement
expressions”
103
Chapter 2
104
Simulation examples
Product Version 10.5
PSpice User's Guide
Part two: Design entry
Part two provides information about how to enter circuit
designs in OrCAD Capture that you want to simulate.
PSpice User's Guide
■
Chapter 3, “Preparing a design for simulation,” 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.
■
Chapter 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 modeling,” describes how
to model analog behavior mathematically or using table
lookups.
■
Chapter 7, “Digital device modeling,” explains the
structure of digital subcircuits and how to create your own
from primitives.
105
Chapter
106
Part two: Design entry
Product Version 10.5
PSpice User's Guide
Preparing a design for
simulation
3
Chapter overview
This chapter provides introductory information to help you
enter circuit designs that simulate properly. If you want an
overview, use the Checklist for simulation setup on page 108
to guide you to specific topics. Refer to the OrCAD Capture
User’s Guide for general schematic entry information.
Topics include:
PSpice User's Guide
■
Checklist for simulation setup on page 108
■
Using parts that you can simulate on page 111
■
Using global parameters and expressions for values on
page 121
■
Defining power supplies on page 133
■
Defining stimuli on page 135
■
Things to watch for on page 140
107
Chapter 3
Preparing a design for simulation
Product Version 10.5
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...
■
Set component
values and other
properties.
See this...
To find out this...
Using parts that you can
simulate on page 111
An overview of vendor, passive,
breakout, and behavioral parts.
Specifying values for part
properties on page 120
Things to consider when
specifying values for part
properties
Using global parameters
and expressions for values
on page 121
How to define values using
variable parameters, functional
calls, and mathematical
expressions.
■
Define power
supplies.
Defining power supplies on An overview of DC power for
page 133
analog circuits and digital power
for mixed-signal circuits.
■
Define input
waveforms.
Defining stimuli on
page 135
An overview of DC, AC, and
time-based stimulus parts.
■
Set up one or more
analyses.
Chapter 8, “Setting up
analyses and starting
simulation”
Procedures, general to all analysis
types, to set up and start the
simulation.
Detailed information about DC,
Chapter 9 through
Chapter 14 (see the table of AC, transient, parametric,
contents)
temperature, Monte Carlo,
sensitivity/worst-case, and digital
analyses.
108
PSpice User's Guide
Product Version 10.5
For more information
on this step...
■
Place markers.
■
Chapter overview
See this...
To find out this...
Using schematic page
markers to add traces on
page 626
How to display results in PSpice by
picking design nets.
Using display control on
page 630
How to limit the data file size.
Advanced design entry and simulation setup steps
For more information See this...
on this step...
■
■
■
Create new
models.
Create new parts.
Choose a
performance
package solution
algorithm.
PSpice User's Guide
To find out how to...
Chapter 4, “Creating and
editing models”
Define models using the Model
Editor or Create Subcircuit Format
Netlist command.
Chapter 6, “Analog
behavioral modeling”
Define the behavior of a block of
analog circuitry as a mathematical
function or lookup table.
Digital device modeling on
page 329
Define the functional, timing, and
I/O characteristics of a digital part.
Chapter 5, “Creating parts
for models”
Create parts either automatically for
models using the part wizard or the
Parts utility, or by manually defining
AKO parts; define
simulation-specific properties.
The OrCAD Capture
User’s Guide
Create and edit part graphics, pins,
and properties in general.
Chapter 8, “Setting up
analyses and starting
simulation”
Choose the solution algorithm that
you want to use. Solver 1 works well
on larger MOS and bipolar circuits
with substantial runtimes.
109
Chapter 3
Preparing a design for simulation
Product Version 10.5
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 information about an error or warning
shown in the Simulation Output window
1
Select the error or warning message.
2
Press F1.
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
Make sure that...
To find out more, see this...
■
The model libraries, stimulus files, and
include files are configured.
Configuring model libraries on page 202
■
The parts you are using have models.
Unmodeled parts on page 140 and Defining
part properties needed for simulation on
page 262
■
You are not using unmodeled pins.
Unmodeled pins on page 145
■
You have defined the grounds.
Missing ground on page 146
■
Every analog net has a DC path to
ground.
Missing DC path to ground on page 146
■
The part template is correct.
Defining part properties needed for simulation
on page 262
■
Hierarchical parts, if used, are properly The OrCAD Capture User’s Guide
defined.
■
Ports that connect to the same net have The OrCAD Capture User’s Guide
the same name.
110
PSpice User's Guide
Product Version 10.5
Using parts that you can simulate
Things to check in your system configuration
Make sure that...
To find out more, see this...
■
Path to the PSpice programs is correct.
■
Directory containing your design has
write permission.
■
Your system has sufficient free memory Your operating system manual
and disk space.
Your operating system manual
Using parts that you can simulate
The PSpice part libraries supply numerous parts designed for
simulation. These include:
■
vendor-supplied parts
■
passive parts
■
breakout parts
■
behavioral parts
The PSpice part libraries also include special parts that you
can use for simulation only. These include:
■
stimulus parts to generate input signals to the circuit
(see Defining stimuli on page 135)
■
ground parts required by all analog and mixed-signal
circuits, which need reference to ground
■
simulation control parts to do things like set bias
values (see Appendix A, “Setting initial state”)
■
output control parts to do things like generate tables
and line-printer plots to the PSpice output file (see
Chapter 19, “Other output options”)
At minimum, a part that you can simulate has these
properties:
■
PSpice User's Guide
A simulation model to describe the part’s electrical
behavior; the model can be:
111
Chapter 3
Preparing a design for simulation
Product Version 10.5
❑
explicitly defined in a model library
❑
built into PSpice
❑
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
The PSpice libraries provide an extensive selection of
manufacturers’ analog and digital 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.
Two types of libraries are provided with PSpice:
■
Standard PSpice libraries
■
PSpice Advanced Analysis libraries
Standard PSpice libraries
The standard PSpice libraries feature over 16,000 analog and
1,600 digital and mixed-signal models of devices
manufactured in North America, Japan, and Europe.
Use parts from standard PSpice libraries or PSpice Advanced
Analysis libraries if you want to analyze the part with PSpice.
112
PSpice User's Guide
Product Version 10.5
Using parts that you can simulate
The standard PSpice libraries are installed at following
locations in the installation directory:
■
Capture symbols for standard PSpice libraries at
\tools\Capture\Library\PSpice\
■
Standard PSpice model libraries at
\tools\PSpice\Library\
The parts in the standard PSpice libraries are listed in the
online PSpice Library List. For information on finding parts
using the online PSpice Library List, see To find parts using
the online library lists on page 116. To find out more about
each model library, read the comments in the .LIB file header.
PSpice Advanced Analysis libraries
The PSpice Advanced Analysis libraries contain over 4,300
analog parts. The Advanced Analysis libraries contain
parameterized and standard parts. The majority of the parts
are parameterized. The parametrized parts have tolerance,
distribution, optimizable and smoke parameters that are
required by the PSpice Advanced Analysis tools. Standard
parts in the Advanced Analysis libraries are similar to parts in
the standard PSpice libraries.
Note: The Advanced Analysis libraries are not available with
PSpice A/D Basics.
The parametrized parts are associated with template-based
PSpice models. An important advantage of using the
template-based PSpice models is that you can pass model
parameters as properties from Capture. For example, if a
template-based model is associated with a part, the model
parameters that you specify on an instance of the part in your
design will be passed to the model. There is no need to edit
the model itself to change a parameter value. This is unlike the
standard PSpice parts that are associated with device
characteristic curve-based PSpice models, where you need to
edit the model to change a simulation parameter. For more
information on template-based and device characteristic
curve-based PSpice models, see Chapter 4, “Creating and
editing models.”
PSpice User's Guide
113
Chapter 3
Preparing a design for simulation
Product Version 10.5
Use parametrized parts from Advanced Analysis libraries if
you want to analyze the part with an Advanced Analysis tool.
Most of the analog parts in the standard PSpice libraries
contain smoke parameters. You can use these parts to
perform smoke analysis using the Smoke tool in PSpice
Advanced Analysis.
This Advanced
Analysis tool...
Uses these part parameters...
Sensitivity
Tolerance parameters
Optimizer
Optimizable parameters
Smoke
Smoke parameters
Monte Carlo
Tolerance parameters,
Distribution parameters
(default parameter value is Flat /
Uniform)
Note: You may use a mixture of standard and parameterized
parts in your design.
The Advanced Analysis libraries are installed at following
locations in the installation directory:
■
Capture symbols for Advanced Analysis libraries at
\tools\Capture\Library\PSpice\AdvAnls\
■
PSpice Advanced Analysis model libraries at
\tools\PSpice\Library
The parts in the Advanced Analysis libraries are listed in the
online PSpice Advanced Analysis Library List. For
information on finding parts using the online PSpice
Advanced Analysis Library List, see To find parts using the
online library lists on page 116. To find out more about each
model library, read the comments in the .LIB file header.
Part naming conventions
The part names in the PSpice libraries usually reflect the
manufacturers’ part names. If multiple vendors supply the
114
PSpice User's Guide
Product Version 10.5
Using parts that you can simulate
same part, each part name includes a suffix that indicates the
vendor that supplied the model.
Example: The PSpice libraries include several models for the
OP-27 opamp as shown by these entries in the online PSpice
Library List.
Notice that there is a generic OP-27 part provided by PSpice,
the OP-27/AD from Analog Devices, Inc., and the OP-27/LT
from Linear Technology Corporation.
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:
PSpice User's Guide
■
the parts browser in Capture and restricting the parts list
to those names that match a specified wildcard text
string, or
■
the online PSpice Library List or the PSpice
Advanced Analysis Library List and searching for the
generic part name using capabilities of the Adobe
115
Chapter 3
Preparing a design for simulation
Product Version 10.5
Acrobat Reader (see To find parts using the online library
lists on page 116).
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:
<wildcard><part_name_fragment><wildcard>
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.
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 PSpice
libraries, such as manufacturer or whether you can simulate it,
then search the online library lists (see To find parts using the
online library lists on page 116).
To find parts using the online library lists
OrCAD provides separate library lists for standard PSpice
libraries and Advanced Analysis libraries. The parts in the
standard PSpice libraries are listed in the online PSpice
Library List. The parts in the Advanced Analysis libraries are
listed in the online PSpice Advanced Analysis Library List.
1
116
Do one of the following:
❑
From the Windows Start menu, choose the Release
OrCAD 10.0 programs folder and then the Online
Documentation shortcut.
❑
From the Help menu in PSpice, choose Manuals.
PSpice User's Guide
Product Version 10.5
Using parts that you can simulate
The Cadence Documentation window appears.
2
Click the PSpice category to show the documents in the
category.
3
Double-click PSpice Library List or PSpice Advanced
Analysis Library List.
This opens the library list in your web browser.
4
Follow the instructions in the second page of the library
list to use the library list.
Note: This method finds only the parts that PSpice supplies
that have models.
If you want to include user-defined parts in the search, use the
parts browser in Capture (see To find parts using the parts
browser on page 116).
Passive parts
The PSpice libraries supply several basic parts based on the
passive device models built into PSpice. These are
summarized in the following table.
Table 3-1 Passive parts
PSpice User's Guide
These parts are
available...
For this device type...
Which is this
PSpice device
letter...
C
C_VAR
capacitor
C
L
inductor
L
R
R_VAR
resistor
R
XFRM_LINEAR
K_LINEAR
transformer
K and L
T
ideal transmission line
T
TLOSSY1
Lossy transmission line T
117
Chapter 3
Preparing a design for simulation
Product Version 10.5
Table 3-1 Passive parts
These parts are
available...
For this device type...
Which is this
PSpice device
letter...
TnCOUPLED2
TnCOUPLEDX2
KCOUPLEn 2
T and K
coupled transmission
line
1. TLOSSY is not available in PSpice A/D Basics packages.
2. For these device types, the PSpice libraries supply several
parts. Refer to the online PSpice Reference Guide for the
available parts.
To find out more about how to use these parts and define their
properties, look up the corresponding PSpice device letter in
the Analog Devices chapter in the online PSpice
Reference Guide, and then see the Capture Parts sections.
Breakout parts
The PSpice libraries supply passive and semiconductor parts
with default model definitions that define a basic set of model
parameters. This way, you can easily:
■
assign device and lot tolerances to model parameters for
Monte Carlo and sensitivity/worst-case analyses.
To find out more about models, see What are models? on
page 151. To find out more about Monte Carlo and
sensitivity/worst-case analyses, see Chapter 13, “Monte
Carlo and sensitivity/worst-case analyses.”
■
define temperature coefficients, and
■
define device-specific operating temperatures.
To find out more about setting temperature parameters,
see the Analog Devices chapter of the online PSpice
Reference Guide and find the device type that you are
interested in.
118
PSpice User's Guide
Product Version 10.5
Using parts that you can simulate
These are called breakout parts and are summarized in the
following table.
Table 3-2 Breakout parts
Use this
breakout part...
For this device
type...
Which is this
PSpice device
letter...
BBREAK
GaAsFET
B
CBREAK
capacitor
C
DBREAKx 1
diode
D
JBREAKx 1
JFET
J
KBREAK
inductor coupling K
LBREAK
inductor
L
MBREAKx 1
MOSFET
M
QBREAKx 1
bipolar transistor Q
RBREAK
resistor
SBREAK
voltage-controlle S
d switch
WBREAK
current-controlle
d switch
R
W
XFRM_NONLINEAR transformer
K and L
ZBREAKN
Z
IGBT
1. For this device type, the PSpice libraries supply several
breakout parts. Refer to the online PSpice Reference
Guide for the available parts.
To find out more about how to use these parts and define their
properties, look up the corresponding PSpice device letter in
the Analog Devices chapter of the online PSpice
Reference Guide, and then look in the Capture Parts
section.
PSpice User's Guide
119
Chapter 3
Preparing a design for simulation
Product Version 10.5
Behavioral parts
Behavioral parts allow you to define how a block of circuitry
should work without having to define each discrete
component.
Analog behavioral parts
These parts use analog behavioral modeling (ABM) to define
each part’s behavior as a mathematical expression or lookup
table. The PSpice 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 tables. You can also create your own
ABM parts. For more information, see Chapter 6, “Analog
behavioral modeling.”
Digital behavioral parts
These parts use special behavioral primitives to define each
part’s functional and timing behavior. These primitives are:
LOGICEXP
PINDLY
CONSTRAINT
to define logic expressions
to define pin-to-pin delays
to define constraint checks
Many of the digital parts provided in the PSpice libraries are
modeled using these primitives. You can also create your own
digital behavioral parts using these primitives.
For more information, see:
■
Chapter 7, “Digital device modeling”
■
the Digital Devices chapter in the online PSpice
Reference Guide.
Specifying values for part properties
Note the following when specifying values for part properties:
120
PSpice User's Guide
Product Version 10.5
Using global parameters and expressions for values
■
Do not leave a space between the value and its unit, if the
unit is a scale symbol. For example, specify 5K instead of
5 K.
For a listing of the scale symbols, see Numeric value
conventions in the Before you begin chapter of the
online PSpice Reference Guide.
■
Do not use the European notation for specifying values.
For example, if you specify 3K3 (the European notation
for 3.3K), PSpice reads the value as 3K. Use 3.3K
instead.
■
Specify tolerance values as percentages. If you specify
an absolute value, the tolerance value will be read as an
absolute number. For example, if you specify the value of
the POSTOL property as a percentage, say 10%, on a
10K resistor, the distribution values will be taken in the
range of 10K ± 1K . If you specify the tolerance value as an
absolute number, say 10, the distribution values will be
taken in the range of 10K ±10Ω .
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
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.
When multiple parts are set to the same value, global
parameters provide a convenient way to change all of their
values for “what-if” analyses. For example, if two independent
sources have a value defined by the parameter VSUPPLY,
then you can change both sources to 10 volts by assigning the
value once to VSUPPLY.
PSpice User's Guide
121
Chapter 3
Preparing a design for simulation
Product Version 10.5
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 variable through 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.
To declare a global parameter
1
Place a PARAM part in your design.
2
Double-click the PARAM part to display the Parts
spreadsheet, then click the New Column or New Row
button.
For more information about using the Parts spreadsheet,
see the OrCAD Capture User’s Guide.
3
To avoid adding the new parameter to the selected filter
for all parts, change the Filter by field to Current
properties.
4
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 (to the right of) the NAMEn
column (or row) and enter a default value for the
parameter.
d. While this cell is still selected, click Display.
122
PSpice User's Guide
Product Version 10.5
Using global parameters and expressions for values
e. In the Display Format frame, select Name and Value,
then click OK.
Note: The system variables in Table 3-5 on page 131 have
reserved parameter names. Do not use these
parameter names when defining your own parameters.
5
Close the Parts spreadsheet.
Example
To declare the global parameter VSUPPLY that will set the
value of an independent voltage source to 14 volts, place the
PARAM part, and then create a new property named
VSUPPLY with a value of 14v.
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.
Example
To set the independent voltage source, VCC, to the value of
the VSUPPLY parameter, set its DC property to {VSUPPLY}.
PSpice User's Guide
123
Chapter 3
Preparing a design for simulation
Product Version 10.5
Expressions
An expression is a mathematical relationship that you can use
to define a numeric or boolean (TRUE/FALSE) value.
PSpice evaluates the expression to a single value every time:
■
it reads in a new circuit, and
■
a parameter value used within an expression changes
during an analysis.
Example: A parameter that changes with each step of a
DC sweep or parametric analysis.
Specifying expressions
To use an expression in your circuit
1
Find the numeric or boolean value you want to replace: a
component value, model parameter value, other property
value, or logic in an IF function test (see Table 3-4 for a
description of the IF function).
2
Replace the value with an expression using the following
syntax:
{ expression }
where expression can contain any of the following:
❑
standard operators listed in Table 3-3
❑
built-in functions listed in Table 3-4
❑
user-defined functions
For more information on user-defined functions, see
the .FUNC command in the Commands chapter in
the online PSpice Reference Guide.
124
❑
system variables listed in Table 3-5
❑
user-defined global parameters
PSpice User's Guide
Product Version 10.5
Using global parameters and expressions for values
For more information on user-defined parameters,
see Using global parameters and expressions for values
on page 121.
❑
literal operands
The curly braces tell PSpice to evaluate the expression
and use its value.
Example
Suppose you have declared a parameter named FACTOR
(with a value of 1.2) and want to scale a -10 V independent
voltage source, VEE, by the value of FACTOR. To do this, set
the DC property of VEE to:
{-10*FACTOR}
PSpice A/D evaluates this expression to:
(-10 * 1.2) or -12 volts
PSpice User's Guide
125
Chapter 3
Preparing a design for simulation
Product Version 10.5
Table 3-3 Operators in expressions
This operator
class...
Includes
this
operator...
arithmetic
+
addition or string
concatenation
-
subtraction
*
multiplication
/
division
**
exponentiation
~
unary NOT
|
boolean OR
^
boolean XOR
&
boolean AND
==
equality test
!=
non-equality test
>
greater than test
>=
greater than or equal to test
<
less than test
<=
less than or equal to test
logical1
relational1
Which means...
1. Logical and relational operators are used within the IF()
function; for digital parts, logical operators are used in
Boolean expressions.
Table 3-4 Functions in arithmetic expressions
This function...
Means this...
ABS(x)
|x|
SQRT(x)
x1/2
ex
EXP(x)
126
PSpice User's Guide
Product Version 10.5
Using global parameters and expressions for values
Table 3-4 Functions in arithmetic expressions, continued
PSpice User's Guide
This function...
Means this...
LOG(x)
ln (x)
which is log base e
LOG10(x)
log (x)
which is log base 10
PWR(x,y)
|x|y
PWRS(x,y)
+|x|y (if x > 0)
-|x|y (if x < 0)
SIN(x)
sin(x)
where x is in radians
ASIN(x)
sin -1 (x)
where the result is in
radians
SINH(x)
sinh (x)
where x is in radians
ASINH(x)
sinh -1 (x)
where x is in radians
COS(x)
cos (x)
where x is in radians
ACOS(x)
cos -1 (x)
where the result is in
radians
COSH(x)
cosh (x)
where x is in radians
ACOSH(x)
cosh -1 (x)
where x is in radians
TAN(x)
tan (x)
where x is in radians
ATAN(x)
ARCTAN(x)
tan -1 (x)
where the result is in
radians
ATAN2(y,x)
tan -1 (y/x)
where the result is in
radians
TANH(x)
tanh (x)
where x is in radians
ATANH(x)
tanh -1 (x)
where x is in radians
M(x)
magnitude of
x1
which is the same as
ABS(x)
P(x)
phase of x1
in degrees; returns 0.0
for real numbers
R(x)
real part of x1
IMG(x)
imaginary part which is applicable to
of x1
AC analysis only
127
Chapter 3
Preparing a design for simulation
Product Version 10.5
Table 3-4 Functions in arithmetic expressions, continued
This function...
Means this...
DDT(x)
time derivative which is applicable to
of x
transient analysis only
Note: In waveform
analysis, this
function is D(x).
SDT(x)
time integral of which is applicable to
x
transient analysis only
Note: In waveform
analysis, this
function is S(x).
TABLE(x,x1,y1,...) y value as a
function of x
MIN(x,y)
minimum of x
and y
MAX(x,y)
maximum of x
and y
where xn,yn point pairs
are plotted and
connected by straight
lines
LIMIT(x,min,max) min if x < min
max if x > max
else x
SGN(x)
+1 if x > 0
0 if x = 0
-1 if x < 0
STP(x)
1 if x >= 0
0 if x < 0
which is used to
suppress a value until a
given amount of time
has passed
Example:
{v(1)*STP(TIME-10ns)}
gives a value of 0.0 until
10 nsec has elapsed,
then gives v(1).
128
PSpice User's Guide
Product Version 10.5
Using global parameters and expressions for values
Table 3-4 Functions in arithmetic expressions, continued
This function...
Means this...
IF(t,x,y)
x if t is true
y otherwise
Zero(expression)
Expression is evluated,
and the function retuirns
the value as 0
I/Ps from kukal
I/Ps from kukal
one(expression)
ceil(arg)
where t is a relational
expression using the
relational operators
shown in Table 3-3
value returned
is an integer
which is either
equal to, or
greater than
the argument
value.
argument should be a
numeric value or an
expression that
evaluates to a numeric
value
Example:
ceil(PI)=4
ceil(5)=5
ceil(5.4)=6
floor(arg)
PSpice User's Guide
value returned
is an integer
which is either
equal to the
argument
value, or is the
nearest
integer,
smaller than
the argument
value.
the argument should be
a numeric value or an
expression that
evaluates to a numeric
value
Example:
floor(PI)=3
floor(5)=5
floor(5.4)=5
129
Chapter 3
Preparing a design for simulation
Product Version 10.5
Table 3-4 Functions in arithmetic expressions, continued
This function...
Means this...
intq(arg)
returns 1, if
arg in an
integer else
returns 0
The argument passed to
this function can be a
numeric value or an
expression that
evaluates to a numeric
value.
1. M(x), P(x), R(x), and IMG(x) apply to Laplace expressions
only.
130
PSpice User's Guide
Product Version 10.5
Using global parameters and expressions for values
The system variables listed in Table 3-5 on page 131, cannot
be used in the trace expressions in the Probe window. These
variables are supported only by the PSpice engine.
Table 3-5 System variables
This
Evaluates to this...
variable...
TEMP
Temperature values resulting from a
temperature, parametric temperature, or DC
temperature sweep analysis.
The default temperature, TNOM, is set in the
Options dialog box (from the Simulation
Settings dialog box, choose the Options tab).
TNOM defaults to 27°C.
Note: TEMP can only be used in expressions
pertaining to analog behavioral modeling
and the propagation delay of digital
models.
Is this note valid after 10.5
enhancements???
Note: If a passive or semiconductor device has
an independent temperature
assignment, then TEMP does not
represent that device’s temperature.
To find out more about customizing
temperatures for passive or semiconductor
devices, refer to the .MODEL command in the
Commands chapter in the online PSpice
Reference Guide.
TIME
Time values resulting from a transient analysis.
If no transient analysis is run, this variable is
undefined.
Note: TIME can only be used in analog
behavioral modeling expressions.
PSpice User's Guide
131
Chapter 3
Preparing a design for simulation
Product Version 10.5
Table 3-5 System variables, continued
This
Evaluates to this...
variable...
RELTOL
Relative tolerance of Voltage and current
The value of this variable is as specified in the
Options tab of the Simulation Settings dialog
box.
ABSTOL
Current tolerance
Describes the best accuracy of currents in a
simulation run. The value of this variable is
specified in the Options tab of the Simulation
Settings dialog box.
VNTOL
Voltage tolerance
Describes the best accuracy of voltages in a
simulation run.The value of this variable is
specified in the Options tab of the Simulation
Settings dialog box.
CHGTOL
Charge tolerance
Describes the best accuracy of charges. The
value of this variable is specified in the Options
tab of the Simulation Settings dialog box.
GMIN
Indicates the minimum conductance used for
any branch. The value of this variable is
specified in the Options tab of the Simulation
Settings dialog box.
Table 3-6 Constants in arithmetic expressions,
Constant..
Value
PI
3.14159265
Validate the value of PI. Upto which decimal point is it
supported.
132
PSpice User's Guide
Product Version 10.5
Defining power supplies
Defining power supplies
For the analog portion of your circuit
If the analog portion of your circuit requires DC power, then
you need to include a DC source in your design. To specify a
DC source, use one of the following parts.
For this source type...
Use this part...
voltage
VDC or VSRC
current
IDC or ISRC
To find out how to use these parts and specify their properties,
see the following:
■
Setting up a DC stimulus on page 423
■
Using VSRC or ISRC parts on page 138
For A/D interfaces in mixed-signal circuits
Default digital power supplies
Every digital part supplied in the PSpice libraries has a default
digital power supply defined for its A-to-D or D-to-A interface
subcircuit. This means that if you are designing a mixed-signal
circuit, then you have a default 5 volt digital power supply
built-in to the circuit at every interface.
Custom digital power supplies
If needed, you can customize the power supply for different
logic families.
PSpice User's Guide
For this logic
family...
Use this part...
CD4000
CD4000_PWR
133
Chapter 3
Preparing a design for simulation
Product Version 10.5
For this logic
family...
Use this part...
TTL
DIGIFPWR
ECL 10K
ECL_10K_PWR
ECL 100K
ECL_100K_PWR
To find out how to use these parts and specify their digital
power and ground pins, see Specifying digital power supplies on
page 583.
134
PSpice User's Guide
Product Version 10.5
Defining power supplies
Defining stimuli
To simulate your circuit, you need to connect one or more
source parts that describe the input signal that the circuit must
respond to.
The PSpice libraries supply several source parts that are
described in the tables that follow. These parts depend on:
■
the kind of analysis you are running,
■
whether you are connecting to the analog or digital
portion of your circuit, and
■
how you want to define the stimulus: using the Stimulus
Editor, using a file specification, or by defining part
property values.
Analog stimuli
Analog stimuli include both voltage and current sources. The
following table shows the part names for voltage sources.
If you want this kind of
input...
Use this part for voltage...
For DC analyses
See Setting up a DC stimulus
on page 423 for more details.
DC bias
VDC or VSRC
For AC analyses
See Setting up an AC stimulus
on page 439 for more details.
AC magnitude and phase
VAC or VSRC
For transient analyses
See Defining a time-based
stimulus on page 474 for more
details.
exponential
PSpice User's Guide
VEXP or VSTIM1
135
Chapter 3
Preparing a design for simulation
Product Version 10.5
If you want this kind of
input...
Use this part for voltage...
periodic pulse
VPULSE or VSTIM1
piecewise-linear
VPWL or VSTIM1
piecewise-linear that repeats VPWL_RE_FOREVER or
forever
VPWL_F_RE_FOREVER2
piecewise-linear that repeats VPWL_N_TIMES or
n times
VPWL_F_N_TIMES2
frequency-modulated sine
wave
VSFFM or VSTIM1
sine wave
VSIN or VSTIM1
1. VSTIM and ISTIM parts require the Stimulus Editor to define
the input signal; these parts are not available in Basics+.
2. VPWL_F_RE_FOREVER and VPWL_F_N_TIMES are
file-based parts; the stimulus specification is saved in a file
and adheres to PSpice netlist syntax.
To determine the part name for an equivalent current
source
−
In the table of voltage source parts, replace the first V in
the part name with I.
For example, the current source equivalent to VDC is
IDC, to VAC is IAC, to VEXP is IEXP, and so on.
Using VSTIM and ISTIM
You can use VSTIM and ISTIM parts to define any kind of
time-based input signal. To specify the input signal itself, you
need to use the Stimulus Editor. See The Stimulus Editor
utility on page 476.
Note: The Stimulus Editor is not included with
PSpice A/D Basics.
136
PSpice User's Guide
Product Version 10.5
Defining power supplies
If you want to specify multiple stimulus types
If you want to run more than one analysis type, including a
transient analysis, then you need to use either of the following:
■
time-based stimulus parts with AC and DC properties
■
VSRC or ISRC parts
Using time-based stimulus parts with AC and DC
properties
The time-based stimulus parts that you can use to define a
transient, DC, and/or AC input signal are listed below.
VEXP
VPULSE
VPWL
VPWL_F_RE_FOREVER
VPWL_F_N_TIMES
VPWL_RE_FOREVER
VPWL_RE_N_TIMES
VSFFM
VSIN
IEXP
IPULSE
IPWL
IPWL_F_RE_FOREVER
IPWL_F_N_TIMES
IPWL_RE_FOREVER
IPWL_RE_N_TIMES
ISFFM
ISIN
In addition to the transient properties, each of these parts also
has a DC and AC property. When you use one of these parts,
you must define all of the transient properties. However, it is
common to leave DC and/or AC undefined (blank). When you
give them a value, the syntax you need to use is as follows.
This property...
Has this syntax...
DC
DC_value[units]
AC
magnitude_value[units]
[phase_value]
For the meaning of transient source properties, refer to the I/V
(independent current and voltage source) device type syntax
in the Analog Devices chapter in the online PSpice
Reference Guide.
PSpice User's Guide
137
Chapter 3
Preparing a design for simulation
Product Version 10.5
Using VSRC or ISRC parts
The VSRC and ISRC parts have one property for each
analysis type: DC, AC, and TRAN. You can set any or all of
them using PSpice netlist syntax. When you give them a
value, the syntax you need to use is as follows.
This property...
Has this syntax...
DC
DC_value[units]
AC
magnitude_value[units]
[phase_value]
TRAN
time-based_type (parameters)
where time-based_type is EXP,
PULSE, PWL, SFFM, or SIN, and the
parameters depend on the
time-based_type.
For the syntax and meaning of
transient source specifications, refer
to the I/V (independent current and
voltage source) device type in the
Analog Devices chapter in the online
PSpice Reference Guide.
Note: If you are running a PSpice-only transient analysis, use
a VSTIM or ISTIM part if you have the standard
package, or one of the other time-based source parts
that has properties specific for a waveform shape.
Digital stimuli
If you want this kind of input...
Use this part....
For transient analyses
138
signal or bus (n width)
DIGSTIMn1
clock signal
DIGCLOCK
1-bit signal
STIM1
4-bit bus
STIM4
PSpice User's Guide
Product Version 10.5
Defining power supplies
If you want this kind of input...
Use this part....
8-bit bus
STIM8
16-bit bus
STIM16
file-based signal or bus (n width)
FILESTIMn
1. The DIGSTIM part requires the Stimulus Editor to
define the input signal; these parts are not available in
PSpice A/D Basics.
You can use the DIGSTIM part to define both 1-bit signal or
bus (n width) input signals using the Stimulus Editor.
See Defining a digital stimulus on page 543 to find out more
about:
PSpice User's Guide
■
all of these source parts, and
■
how to use the Stimulus Editor to specify DIGSTIMn
(DIGSTIM1, DIGSTIM4, etc.) part.
139
Chapter 3
Preparing a design for simulation
Product Version 10.5
Things to watch for
This section includes troubleshooting tips for some of the most
common reasons your circuit design may not netlist or
simulate.
For a roadmap to other commonly encountered problems and
solutions, see When netlisting fails or the simulation does not
start on page 110.
Unmodeled parts
If you see messages like this in the PSpice Simulation Output
window,
Warning: Part part_name has no simulation model.
then you may have done one of the following things:
■
Placed a part from the PSpice libraries that is not
available for simulation (used only for board layout).
■
Placed a custom part that has been incompletely defined
for simulation.
Do this if the part in question is from the PSpice libraries
■
Replace the part with an equivalent part from one of the
libraries listed in the tables below.
■
Make sure that you can simulate the part by checking the
following:
❑
That it has a PSPICETEMPLATE property and that
its value is non-blank.
The libraries listed in the tables that follow all contain
parts that you can simulate. Some files also contain
parts that you can only use for board layout. That’s
why you need to check the PSPICETEMPLATE
property if you are unsure or still getting warnings
when you try to simulate your circuit.
140
PSpice User's Guide
Product Version 10.5
Defining power supplies
❑
That it has an Implementation Type = PSpice
MODEL property and that its Implementation
property is non-blank.
Note: The PSPICETEMPLATE property is case insensitive,
and is shown throughout the documentation in capital
letters by convention only.
PSpice User's Guide
141
Chapter 3
Preparing a design for simulation
Product Version 10.5
Table 3-7
Analog libraries with modeled parts (installed in
\tools\Capture\Library\PSpice)
1_SHOT
EPWRBJT
ON_AMP
ABM
FAIRCHILD
ON_BJT
ADV_LIN
FILTSUB
ON_DIODE
AMP
FWBELL
ON_MOS
ANALOG
HARRIS
ON_PWM
ANA_SWIT
IBGT1
OPAMP
ANLG_DEV
INFINEON
OPTO
ANL_MISC
IXYS
PHIL_BJT
APEX
JBIPOLAR
PHIL_DIODE
APEX_PWM
JDIODE
PHIL_FET
BIPOLAR
JFET
PHIL_RF
BREAKOUT
JJFET
POLYFET
BUFFER
JOPAMP
PWRBJT
BURR_BRN
JPWRBJT
PWRMOS
CD4000
JPWRMOS
SWIT_RAV
COMLINR
LINEDRIV
SWIT_REG
DATACONV
LIN_TECH
TEX_INST
DARLNGTN
MAGNETIC1
THYRISTR1
DIODE
MAXIM
TLINE1
EBIPOLAR
MIX_MISC2
XTAL
EDIODE
MOTORSEN
ZETEX
ELANTEC
MOTOR_RF
EPCOS
NAT_SEMI
1. Not included in PSpice A/D Basics.
2. Contains mixed-signal parts.
142
PSpice User's Guide
Product Version 10.5
Defining power supplies
Digital libraries with modeled parts
7400
74H
DIG_ECL
74AC
74HC
DIG_GAL
74ACT
74HCT
DIG_MISC
74ALS
74L
DIG_PAL
74AS
74LS
DIG_PRIM
74F
74S
To find out more about a particular library, refer to the online
PSpice Library List or read the header of the model library
file itself.
Check for this if the part in question is custom-built
Are there blank (or inappropriate) values for the part’s
Implementation and PSPICETEMPLATE properties?
If so, load this part into the part editor and set these properties
appropriately. One way to approach this is to edit the part that
appears in your design.
To edit the properties for the part in question
1
In the schematic page editor, select the part.
2
From the Edit menu, choose Part.
The part editor window appears with the part already
loaded.
3
From the Edit menu, choose Properties and proceed to
change the property values.
To find out more about setting the simulation properties for
parts, see Defining part properties needed for simulation on
page 262. To find out more about using the part editor, refer to
your OrCAD Capture User’s Guide.
PSpice User's Guide
143
Chapter 3
Preparing a design for simulation
Product Version 10.5
Unconfigured model, stimulus, or include files
If you see messages like these in the PSpice Simulation
Output window,
(design_name) Floating pin: refdes pin pin_name
Floating pin: pin_id
File not found
Can’t open stimulus file
or messages like these in the PSpice output file,
Model model_name used by device_name is undefined.
Subcircuit subckt_name used by device_name is
undefined.
Can’t find .STIMULUS “refdes” definition
then you may be missing a model library, stimulus file, or
include file from the configuration list, or the configured file is
not on the library path.
Check for this
■
Does the PSpice library configuration file NOM.LIB
appear in the Library files list in the Configuration Files
tab in the Simulation Profile?
■
Does the relevant model library, stimulus file, or include
file appear in the configuration list?
■
If the file is configured, does the default library search
path include the directory path where the file resides, or
explicitly define the directory path in the configuration
list?
If the file is not configured, add it to the list and make sure that
it appears before any other library or file that has an
identically-named definition.
To find out more about how to configure these files and about
search order, see Configuring model libraries on page 202. To
find out more about the default configuration, see How are
models organized? on page 152.
144
PSpice User's Guide
Product Version 10.5
Defining power supplies
To view the configuration list
1
In the Simulation Settings dialog box, click the
Configuration Files tab and view the Library, Include, and
Stimulus files lists.
If the directory path is not specified in each, update the
default library search path or change the file entry in the
configuration list to include the full path specification.
To view the default library search path
1
In the Simulation Settings dialog box, click the
Configuration Files tab.
2
Click Library in the Category field to display the Library
files list.
To find out more about the library search path, see Changing
the library search path on page 210.
Unmodeled pins
If you see messages like these in the PSpice Simulation
Output window,
Warning: Part part_name pin pin_name is unmodeled.
Warning: Less than 2 connections at node node_name.
or messages like this in the PSpice output file,
Floating/unmodeled pin fixups
then you may have drawn a wire to an unmodeled pin.
The PSpice libraries include parts that are suitable for both
simulation and board layout. The unmodeled pins map into
packages but have no electrical significance; PSpice ignores
unmodeled pins during simulation.
Check for this
Are there connections to unmodeled pins?
If so, do one of the following:
PSpice User's Guide
145
Chapter 3
Preparing a design for simulation
Product Version 10.5
■
Remove wires connected to unmodeled pins.
■
If you expect the connection to affect simulation results,
find an equivalent part that models the pins in question
and draw the connections. To find out more about
searching for parts, see Finding the part that you want on
page 115.
Missing ground
This problem applies to analog-only and mixed-signal circuits.
If for every net in your circuit you see this message in the
PSpice output file,
ERROR -- Node node_name is floating.
then your circuit may not be tied to ground.
Check for this
Are there ground parts named 0 (zero) connected
appropriately in your design?
If not, place and connect one (or more, as needed) in your
design. You can use the 0 (zero) ground part in SOURCE.OLB
or any other ground part as long as you change its name to 0.
Missing DC path to ground
This problem applies to analog-only and mixed-signal circuits.
If for selected nets in your circuit you see this message in the
PSpice output file,
ERROR -- Node node_name is floating.
then you may be missing a DC path to ground.
Check for this
Are there any nets that are isolated from ground by either
open circuits or capacitors?
146
PSpice User's Guide
Product Version 10.5
Defining power supplies
If so, then add a very large (for example, 1 Gohm) resistor
either:
■
in parallel with the capacitor or open circuit, or
■
from the isolated net to ground.
Note: When calculating the bias point solution, PSpice treats
capacitors as open circuits and inductors as short
circuits.
Example: The circuit shown below connects capacitors (DC
open circuits) such that both ends of inductor L2 are isolated
from ground.
When simulated, PSpice A/D flags nets 2 and 3 as floating.
The following topology solves this problem.
PSpice User's Guide
147
Chapter 3
148
Preparing a design for simulation
Product Version 10.5
PSpice User's Guide
Creating and editing models
4
Chapter overview
This chapter provides information about creating and editing
models for parts that you want to simulate.
Topics are grouped into four areas introduced later in this
overview. If you want to find out quickly which tools to use to
complete a given task and how to start, then:
1
Go to the roadmap in Ways to create and edit models on
page 161.
2
Find the task you want to complete.
3
Go to the sections referenced for that task for more
information about how to proceed.
Background information
These sections present model library concepts and an
overview of the tools that you can use to create and edit
models:
PSpice User's Guide
■
What are models? on page 151
■
How are models organized? on page 152
■
Tools to create and edit models on page 160
149
Chapter 4
Creating and editing models
Product Version 10.5
Task roadmap
This section helps you find other sections in this chapter that
are relevant to the model editing task that you want to
complete:
■
Ways to create and edit models on page 161
How to use the tools
These sections explain how to use different tools to create and
edit models on their own and when editing schematic pages
or parts:
■
For a list of device types that the Model Editor supports,
see Table 4-2 and Table 4-3. If the Model Editor does not
support the device type for the model definition that you
want to create, then you can use a standard text editor to
create a model definition using the PSpice .MODEL and
.SUBCKT command syntax. Remember to configure the
new model library (see Configuring model libraries on
page 202).
■
Editing model text on page 193
■
Using the Create Subcircuit Format Netlist command on
page 196
Other useful information
These sections explain how to configure and reuse models
after you have created or edited them:
150
■
Changing the model reference to an existing model
definition on page 199
■
Reusing instance models on page 200
■
Configuring model libraries on page 202
PSpice User's Guide
Product Version 10.5
Chapter overview
What are models?
A model defines the electrical behavior of a part. On a
schematic page, this correspondence is defined by the
Implementation property on the part, which is assigned the
model name.
Depending on the device type that it describes, a model is
defined as one of the following:
■
a model parameter set
■
a subcircuit netlist
Both ways of defining a model are text-based, with specific
rules of syntax.
Models defined as model parameter sets
PSpice has built-in algorithms or models that describe the
behavior of many device types. The behavior of these built-in
models is described by a set of model parameters.
You can define the behavior for a device that is based on a
built-in model by setting all or any of the corresponding model
parameters to new values using the PSpice .MODEL syntax.
For example:
.MODEL MLOAD NMOS
+ (LEVEL=1 VTO=0.7 CJ=0.02pF)
Note: In addition to the analog models built into PSpice, the
.MODEL syntax applies to the timing and I/O
characteristics of digital parts.
Models defined as subcircuit netlists
For some devices, there are no PSpice built-in models that
can describe their behavior fully. These types of devices are
defined using the PSpice .SUBCKT/.ENDS or subcircuit
syntax instead.
Subcircuit syntax includes:
■
PSpice User's Guide
Netlists to describe the structure and function of the part.
151
Chapter 4
Creating and editing models
■
Product Version 10.5
Variable input parameters to fine-tune the model.
For example:
* FIRST ORDER RC STAGE
.SUBCKT LIN/STG IN OUT AGND
+ PARAMS: C1VAL=1 C2VAL=1 R1VAL=1 R2VAL=1
+
GAIN=10000
C1 IN N1
{C1VAL}
C2 N1 OUT {C2VAL}
R1 IN N1
{R1VAL}
R2 N1 OUT {R2VAL}
EAMP1 OUT AGND VALUE={V(AGND,N1)*GAIN}
.ENDS
To find out more about PSpice command and netlist syntax,
refer to the online PSpice Reference Guide.
How are models organized?
The key concepts behind model organization are as follows:
■
Model definitions are saved in files called model libraries.
■
Model libraries must be configured so that PSpice
searches them for definitions.
■
Depending on the configuration, model libraries are
available either to a specific profile, to a specific design or
to all (global) designs. For more information, see Global
vs. design vs. profile models and libraries on page 153.
Model libraries
Device model and subcircuit definitions are organized into
model libraries. Model libraries are text files that contain one
or more model definitions. Typically, model library names have
a .LIB extension.
Most model libraries contain models of similar type. For
vendor-supplied models, libraries are also partitioned by
manufacturer. For example, MOTOR_RF.LIB contains models
for Motorola-made RF bipolar transistors.
To find out more about the models contained in a model
library, read the comments in the file header.
152
PSpice User's Guide
Product Version 10.5
How are models organized?
Note: You can use the PSpice Model Editor, or any standard
text editor, to view model definitions in libraries.
Model library configuration
PSpice searches model libraries for the model names
specified by the MODEL implementation for parts in your
design. These are the model definitions that PSpice uses to
simulate your circuit.
For PSpice to locate these model definitions, you must
configure the libraries. This means:
■
Specifying the directory path or paths to the model
libraries.
■
Naming each model library that PSpice should search
and listing them in the desired search order.
■
Assigning global, design or profile scope to the model
library.
To optimize the model library search, PSpice uses indexes. To
find out more about this and how to add, delete, and rearrange
configured libraries, see Configuring model libraries on
page 202.
Global vs. design vs. profile models and libraries
Model libraries and the models they contain have either
profile, design or global application to your designs.
Profile models
Profile models apply to one profile. You can create models
using the Model Editor and then manually configure the new
libraries for a specific profile.
Example usage: To set up device and lot tolerances on the
model parameters for a particular part instance when running
a Monte Carlo or sensitivity/worst-case analysis using a
specific profile.
PSpice User's Guide
153
Chapter 4
Creating and editing models
Product Version 10.5
Design models
Design models apply to one design. The schematic page
editor automatically creates a design model whenever you
modify the model definition for a part instance on your
schematic page. You can also create models externally and
then manually configure the new libraries for a specific design.
Example usage: To set up device and lot tolerances on the
model parameters for a particular part instance when running
a Monte Carlo or sensitivity/worst-case analysis.
Global models
Global models are available to all designs you create. The
part editor automatically creates a global model whenever
you create a part with a new model definition. The Model
Editor also creates global models. You can also create models
externally and then manually configure the new libraries for
use in all designs.
To find out how to change the profile, design and global
configuration of model libraries, see Changing the model
library scope from profile to design, profile to global, design to
global and vice versa on page 206.
PSpice searches profile libraries before design libraries and
design libraries before global libraries. To find out more, see
Changing model library search order on page 208.
Nested model libraries
Besides model and subcircuit definitions, model libraries can
also contain references to other model libraries using the
PSpice .LIB syntax. When searching model libraries for
matches, PSpice also scans these referenced libraries.
Example: Suppose you have two custom model libraries,
MYDIODES.LIB and MYOPAMPS.LIB, that you want
PSpice A/D to search any time you simulate a design. Then
you can create a third model library, MYMODELS.LIB, that
contains these two statements:
154
PSpice User's Guide
Product Version 10.5
How are models organized?
.LIB mydiodes.lib
.LIB myopamps.lib
and configure MYMODELS.LIB for global use. Because
MYDIODES.LIB and MYOPAMPS.LIB are referenced from
MYMODELS.LIB, they are automatically configured for global
use as well.
PSpice-provided models
The model libraries that you initially install with your PSpice
programs are listed in NOM.LIB. This file demonstrates how
you can nest references to other libraries and models.
If you click the Configuration Files tab in the Simulation
Settings dialog box and view the Library files list immediately
after installation, you see the
NOM.LIB entry in the Library
files list. The
icon means that this model library and any of
the model libraries it references contain global model
definitions.
Model library data
Information contained in PSpice model libraries can be
classified as:
■
Simulation information
■
Device information
Simulation information
Simulation information is also termed as model information
and is used while simulating the models. Depending on the
method of creation, PSpice simulation models are of two
types:
PSpice User's Guide
■
Device characteristic curves-based models
■
Template-based models
155
Chapter 4
Creating and editing models
Product Version 10.5
Device characteristic curves-based models
Simulation models based on the device characteristic curves
are the models that are historically being used in the
Capture-PSpice flow. You can extract device parameters
based on the device characteristic curves in the data sheets.
For a list of device characteristic curve-based models
provided with PSpice, refer to the online PSpice Library List.
Template-based models
These simulation models are based on PSpice-provided
templates and are a new addition to the PSpice model library.
Simulation models that are based on PSpice provided
templates are also referred to as parameterized models.
Parameterized models are specified in terms of model
parameters. Changing a parameter changes the behavior of
the model. Template-based PSpice models describe the
analog simulation behavior of a device in terms of parametric
equations. These models are of the .SUBCKT type. The
.SUBCKT wrapper enables symbol properties to be passed as
parameters to the simulator.
The PSpice-provided templates are available in the
TEMPLATES.LIB file. This is an encrypted file, and
template-based models are wrappers to this file.
The main advantage of using template-based models is that
simulation parameter values can be passed as properties
from Capture. Besides this, parameterized models are best
suited to be used with PSpice Advanced Analysis, and also for
performing statistical analysis for variations in model
parameters.
For a list of template-based device models provided with
PSpice, refer to the online PSpice Advanced Analysis
Library List.
For a description of models supported by the Model Editor,
see Model Editor-supported device types based on PSpice
templates on page 173.
156
PSpice User's Guide
Product Version 10.5
How are models organized?
Device information
Information that is specific to each device, such as simulation
parameter tolerance and maximum operating conditions, is
termed as device information. The device information is stored
in the device property file and is required by PSpice Advanced
Analysis. To know more about the device property file, see
Appendix A, Property Files in the PSpice Advanced
Analysis User’s Guide.
You can use the Model Editor to add device information to a
model. For template-based simulation models, you can add
smoke and tolerance information. For other simulation
models, you can add only the smoke information.
Tolerance information is required to perform a Monte Carlo
and Sensitivity/Worst-Case analysis. To know more about
Monte Carlo and Sensitivity/Worst-Case analysis, see
PSpice Advanced Analysis User’s Guide.
The tolerance information is added in the Simulation
Parameters frame but smoke information can be added or
modified only if you have Advanced Analysis installed. See
Adding tolerance information on page 172
To know more about how to add smoke information to a model
using the Model Editor, see Handling smoke information using
the Model Editor on page 212.
Device characteristic curves-based models vs. Template-based models
Table 4-1 highlights the differences between two types of
simulation models.
Table 4-1 Differences between device characteristic curves-based and
template-based models
Device characteristic curves-based
PSpice models
Template-based PSpice models
They are based on device characteristic
curves. Device characteristic curves can be
obtained from device datasheets.
They are based on PSpice-provided
templates.
PSpice User's Guide
157
Chapter 4
Creating and editing models
Product Version 10.5
Table 4-1 Differences between device characteristic curves-based and
template-based models
Device characteristic curves-based
PSpice models
Template-based PSpice models
They cannot be used for Advanced Analysis They can be used for all Advanced Analysis
Sensitivity, Monte Carlo, and Optimizer runs. runs, such as Sensitivity, Smoke, Monte
They can be used for Advanced Analysis
Carlo, and Optimizer.
smoke test only if smoke information is
explicitly added.
All simulation information is contained in the Models are wrappers to a template model
model itself.
file. Therefore, both the model and the
template model are required for simulation.
The PSpiceTemplate property must be
attached to the symbol for generating the
PSpice netlist.
To know more about the PSpiceTemplate
property, see PSPICETEMPLATE on
page 263.
The PSpiceTemplate property is not required
on the symbol. The PORT_ORDER
information present in the device property
file is used for generating the PSpice netlist.
Note: The model library and the device
property file must have the same
name and must be at the same
location.
To know more about the device property file,
see Appendix A, Property Files in the
PSpice Advanced Analysis User’s
Guide.
Simulation parameter values can be passed
as properties from the schematic editor. This
implies that instance-specific values of
simulation parameters can be passed from
the schematic editor, without changing the
To know more, see Using the Model Editor to original model.
edit the D1 diode model on page 182.
To know more, see Changing the level for
CA1458 on page 249.
To modify a simulation property, you need to
edit the simulation parameter. This implies
that you either update the values in the
original model or create an instance model
for the design.
158
PSpice User's Guide
Product Version 10.5
How are models organized?
Table 4-1 Differences between device characteristic curves-based and
template-based models
Device characteristic curves-based
PSpice models
Template-based PSpice models
By default, tolerance and smoke information Tolerance and smoke information for the
is not available in the models created using device is available in the device property file
the Model Editor.
associated with the model library.
Editing model text to add DEV and LOT
information does not make the model
compatible with Advanced Analysis Monte
Carlo run.
If PSpice Advanced Analysis is installed,
default values for the smoke parameters are
visible through the Model Editor user
interface.
Note: The shape and size of the part symbol generated by the Model Editor for the
template-based models and device characteristic curves-based models may be
different.
PSpice User's Guide
159
Chapter 4
Creating and editing models
Product Version 10.5
Tools to create and edit models
There are two tools that you can use to create and edit model
definitions.
■
The Model Editor
Use the Model Editor when you want to:
❑
derive models from data sheet curves provided by
manufacturers.
❑
create models based on PSpice-provided templates.
❑
modify the behavior of a Model Editor-supported
model.
❑
edit the PSpice command syntax (text) for .MODEL
and .SUBCKT definitions.
Note: For template-based models, the model text is
read-only and cannot be edited using the Model Editor.
Note: The Model Editor is not available with PSpice. A
limited version of the Model Editor is supplied with
PSpice A/D Basics.
■
Capture
Use the Create Subcircuit Format Netlist command in
Capture when you have a hierarchical level in your design
that you want to set up as an equivalent part with behavior
described as a subcircuit netlist (.SUBCKT syntax).
Note: The Create Subcircuit Format Netlist command
does not help you create a hierarchical design. You need
to create this yourself before using the Create Subcircuit
Format Netlist command. For information on hierarchical
designs and how to create them, refer to the OrCAD
Capture User’s Guide.
Note: If you created a subcircuit definition using the
Create Subcircuit Format Netlist command and want to
alter it, use the Model Editor to edit the definition, or
modify the original hierarchical schematic and run Create
Subcircuit Format Netlist again to replace the definition.
160
PSpice User's Guide
Product Version 10.5
How are models organized?
Ways to create and edit models
This section is a roadmap to other information in this chapter.
Find the task that you want to complete, then go to the
referenced sections for more information.
If you want to...
■
Create a model
from scratch and
automatically create a
symbol for it to use in
any schematic.
■
Create a model
from scratch
without a symbol
and have the model
definition available to
any design.
■
View model
characteristics for a
part.
Create a new
model by copying
an existing model
■
Then do this...
Running the Model Editor
Start the Model Editor and
alone on page 165.
enable/disable automatic
symbol creation as needed.
Then, create or view the model.
Copy the text of an existing
model in a text editor and
rename the file.
or
From the Model menu, choose
the Copy From command.
■
Create or edit the
model for an
existing symbol
and incorporate the
changes in all
schematics that use
that symbol.
PSpice User's Guide
To find out more, see this...
Model Editor Help
First, create or load the symbol
in Capture, and then edit the
model using the Model Editor.
You can edit models by:
■
changing parameter
values in the Parameters
window.
■
editing text in the Model
Text window.
Running the Model Editor from
the schematic editor on
page 177.
Editing model text on
page 193
161
Chapter 4
Creating and editing models
If you want to...
■
Then do this...
Product Version 10.5
To find out more, see this...
Edit a model to add Start the Model Editor and
smoke information.
open the library with the model,
and then add the smoke
information.
Note: This feature is available
only if you have
Advanced Analysis
installed on your
machine.
■
Define tolerances Select the part instance on
Editing model text on
on model parameters your schematic and then edit
page 193.
for statistical analysis. the model text using the Model
Editor.
Note: For template-based
PSpice models,
tolerance information
can be added in the
Postol and Negtol
columns of the
Simulation Parameters
window.
■
■
■
Test behavior
Select the part instance on
variations on a part. your schematic and then edit
the model using either:
Refine a model
■
the Model Editor, or
before making it
available to all
■
editing the Model Text in a
schematics.
text editor.
Derive subcircuit
definitions from a
hierarchical
schematic.
Running the Model Editor from
the schematic editor on
page 177.
Starting the Model Editor on
page 178.
In the Project Manager, select Using the Create Subcircuit
Format Netlist command on
the .DSN file. From the Tools
menu, choose Create Netlist, page 196.
select the PSpice tab, and then
check the Create Subcircuit
Format Netlist check box.
Note: For a list of device types that the Model Editor supports,
see Table 4-2 and Table 4-3. If the Model Editor does
not support the device type for the model definition that
162
PSpice User's Guide
Product Version 10.5
Using the Model Editor
you want to create, then you can use a standard text
editor to create a model definition using the PSpice
.MODEL and .SUBCKT command syntax. Remember
to configure the new model library (see Configuring
model libraries on page 202).
Using the Model Editor
The Model Editor converts information that you enter from the
device manufacturer’s data sheet into either:
■
model parameter sets using PSpice .MODEL syntax, or
■
subcircuit netlists using PSpice .SUBCKT syntax.
Note: The Extract Model view in the Model Editor does
not support the following subcircuit constructs:
❑
optional nodes construct, OPTIONAL:
❑
variable parameters construct, PARAMS:
❑
local .PARAM command
❑
local .FUNC command
To refine the subcircuit definition for these constructs, use
the Model Text view in Model Editor, described in Editing
model text on page 193.
The Model Editor then saves these definitions to model
libraries that PSpice can search when looking for simulation
models.
model libraries
OrCAD
Capture
Model Editor
model
definitions
PSpice User's Guide
PSpice A/D
exported
model file
163
Chapter 4
Creating and editing models
Product Version 10.5
Figure 4-1 Relationship of the Model Editor to Capture
and PSpice.
Note: By default, the Model Editor creates or updates model
libraries. To create an exported model file, choose the
Export command from the Model menu and configure
it as an include file. For more information, see How
PSpice uses model libraries on page 203.
Note: The Model Editor is not available with PSpice. A limited
version of the Model Editor is supplied with
PSpice A/D Basics.
Ways to use the Model Editor
You can use the Model Editor in the following ways:
■
To define a new model, and then automatically
create a part. Any new models and parts are
automatically available to any design. To find out more,
see Running the Model Editor alone on page 165.
■
To define a new model only (no part). You can
optionally turn off the part creation feature for new
models. The model definition is available to any design,
for example, by changing the model implementation for a
part instance. To find out more, see Running the Model
Editor alone on page 165.
■
To edit a model definition for a part instance on
your schematic. This means you need to start the
Model Editor from the schematic editor after selecting a
part instance on your schematic. The schematic editor
automatically attaches the new model implementation
(that the Model Editor creates) to the selected part
instance. To find out more, see Running the Model Editor
from the schematic editor on page 177.
■
To examine or verify the electrical characteristics
of a model without running PSpice. This means you
can use the Model Editor alone to:
❑
164
check characteristics of a model quickly, given a set
of model parameter values, or
PSpice User's Guide
Product Version 10.5
Running the Model Editor alone
❑
compare characteristic curves to data sheet
information or measured data.
To find out more, see Running the Model Editor alone on
page 165.
■
To add and modify a model definition for
parameterized or template-based PSpice models.
This means you can create new parameterized models.
You can also edit the existing models in the
parameterized libraries to modify the values of simulation
parameters.
■
Adding and editing smoke data to the models supported
by the Model Editor. If you have Advanced Analysis
installed on your machine, you can use the Model Editor
to add smoke information to device characteristic
curves-based PSpice models. Editing of smoke
information is possible for all types of PSpice models.
Running the Model Editor alone
Run the Model Editor alone if you want to do any of the
following:
■
create a model and use the model in any design (and
automatically create a part),
■
create a model and have the model definition available to
any design (without creating a part), or
■
examine or verify the characteristics of a given model
without using PSpice.
Running the Model Editor alone means that the model you are
creating or examining is not currently tied to a part instance on
your schematic page or to a part editing session.
Note: You can edit models in the Edit Model View only for
device types that the Model Editor supports.
PSpice User's Guide
165
Chapter 4
Creating and editing models
Product Version 10.5
Starting the Model Editor
To start the Model Editor alone
1
From the Start menu, point to Programs, Release OrCAD
10.0, choose PSpice Accessories and then choose
Model Editor.
2
From the File menu, choose New or Open.
If you have already started the Model Editor from Capture and
want to continue working on new models, then:
1
Save the opened model library.
2
Open or create a different model library.
3
Get a model, or create a new one.
Creating models using the Model Editor
Using the Model Editor, you can create models from scratch.
The Model Editor supports creation of PSpice models based
on device characteristic curves as well as templates. This
section covers:
■
Creating models based on device characteristic curves
■
Creating models based on PSpice templates
Creating models based on device characteristic curves
1
In the Model Editor, open a library.
2
From the Models menu, choose New.
3
Specify the name of the new model in the Model Name
text box.
4
Select the Use Device Characteristic Curves option.
5
From the From Model drop-down list, select the device
type and click OK.
Note: Depending of the device type, you may have to
166
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
provide some other details. For example, if the device
type is Bipolar Transistor, you will also need to specify if
the BJT will be of NPN or PNP type.
All the device characteristic curves for the device and the
simulation parameters are displayed. You can now
characterize the models by either using data sheets or
editing simulation parameter values.
Ways to characterize models
Figure 4-2 shows two ways to characterize PSpice models
using the Model Editor.
device data from
data sheets
parts
estimation
model
parameters
PSpice A/D
simplified
equation
evaluation
graph of device
characteristic
user
data-entry
“what-if” model data
Figure 4-2 Process and data flow for the Model Editor
Testing and verifying models created with the Model
Editor
Each curve in the Model Editor is defined only by the
parameters being adjusted. For the diode, the forward current
curve only shows the part of the current equation that is
PSpice User's Guide
167
Chapter 4
Creating and editing models
Product Version 10.5
associated with the forward characteristic parameters (such
as IS, N, Rs).
However, PSpice uses the full equation for the diode model,
which includes a term involving the reverse characteristic
parameters (such as ISR, NR). These parameters could have
a significant effect at low current.
This means that the curve displayed in the Model Editor does
not exactly match what is displayed in PSpice after a
simulation. Be sure to test and verify models using PSpice. If
needed, fine-tune the models.
Creating models from data sheet information
The most common way to characterize models is to enter data
sheet information for each device characteristic. After you are
satisfied with the behavior of each characteristic, you can
have the Model Editor estimate (or extract) the corresponding
model parameters and generate a graph showing the behavior
of the characteristic. This is called the fitting process.
You can repeat this process, and when you are satisfied with
the results, save them; the Model Editor creates model
libraries containing appropriate model and subcircuit
definitions.
Note: When specifying operating characteristics for a model,
you can use typical values found on data sheets
effectively for most simulations. To verify your design,
you may also want to use best- and worst-case values
to create separate models, and then swap them into the
circuit design.
Analyzing the effect of model parameters on device
characteristics
You can also edit model parameters directly and see how
changing their values affects a device characteristic. As you
change model parameters, the Model Editor recalculates the
behavior of the device characteristics and displays a new
curve for each of the affected ones.
168
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
How to fit models
For a given model, the Model Editor displays a list of the
device characteristics and a list of all model parameters and
performance curves (see Figure 4-3).
For more information about the characteristics of devices
supported by the Model Editor, refer to the online PSpice
Reference Guide.
Figure 4-3 Model Editor workspace with data for a bipolar
transistor.
To fit the model
1
For each device characteristic that you want to set up:
a. In the Spec Entry frame, click the tab of the device
characteristic.
b. Enter the device information from the data sheet.
2
From the Tools menu, choose Extract Parameters to
extract all relevant model parameters for the current
specification.
A check mark appears in the Active column of the
Parameters frame for each extracted model parameter.
PSpice User's Guide
169
Chapter 4
Creating and editing models
Product Version 10.5
To keep a parameter value fixed, check the Fixed field
corresponding to the parameter.
3
Repeat steps 1-2 until the model meets target behaviors.
To view updated performance curves
1
On the toolbar, click the Update Graph button
.
Note: If you view performance curves before fitting, then your
data points and the curve for the current model
specification may not match.
Model Editor-supported device types based on device characteristic curves
Device types that the Model Editor models using the .MODEL
statement are based on the models built into PSpice.
Table 4-2 summarizes the device types for which you can
create PSpice models based on characteristic curves.
Table 4-2 Device characteristic curves-based device
types supported in Model Editor
170
This part type...
Uses this
definition
form...
And this
name
prefix1...
diode2
.MODEL
D
bipolar transistor
.MODEL
Q
bipolar transistor, Darlington
model
.SUBCKT
X
IGBT
.MODEL
Z
JFET
.MODEL
J
MOSFET
.MODEL
M
operational amplifier3
voltage comparator
.SUBCKT
X
.SUBCKT
X
voltage regulator
.SUBCKT
X
voltage reference
.SUBCKT
X
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
Table 4-2 Device characteristic curves-based device
types supported in Model Editor
This part type...
Uses this
definition
form...
And this
name
prefix1...
magnetic core4
.MODEL
K
1. This is the standard PSpice device letter notation. Refer to the
online PSpice Reference Guide.
2. The part type DIODE is the only part supported in PSpice A/D
Basics.
3. Model Editor supports only .SUBCKT models that were
created using the Model Editor. However, you can edit the text
of a .SUBCKT model created manually or by another tool
using the Model Editor. When you load a .SUBCKT model that
the Model Editor did not create, the Model Editor displays the
text of the model for editing.
4. To find out more about Magnetic Core models, see PSpice
Reference Manual.
Note: The model parameter defaults used by the Model
Editor are different from those used by the models built
into PSpice.
Creating models based on PSpice templates
An important advantage of using the template-based PSpice
models is that you can pass simulation parameters as
properties from the schematic editor. This implies that you can
have instance-specific values for the model parameters. To
know more about passing parameter values as properties
from the schematic editor, see Changing the level for CA1458
on page 249.
For a description of template-based models supported by the
Model Editor, see Model Editor-supported device types based
on PSpice templates on page 173.
To create a template-based PSpice model, complete the
following steps.
1
PSpice User's Guide
In Model Editor, create a new library or open an existing
library.
171
Chapter 4
Creating and editing models
Product Version 10.5
2
From the Model menu, choose New.
3
Specify the name of the new model in the Model Name
text box.
4
Select the Use Templates option.
5
From the From Model drop-down list, select the device
type.
Depending of the device type, you may have to provide
some other details. For example, if the device type is
Bipolar Transistor, you will also need to specify if the BJT
will be of NPN or PNP type.
6
Click OK.
The Simulation parameters window appears with the
default values of all simulation parameters. These values
are editable and can be modified as required.
Notice that the Model Text window of a template-based
PSpice model is not editable, it is read-only. Also, the
model text does not display the port information under the
.SUBCKT statement.
Adding tolerance information
While creating template-based simulation models, you can
add tolerance information using the Model Editor user
interface. Tolerance information is required only for Advanced
Analysis Monte Carlo and Sensitivity runs and not for
simulating the models.
The Postol, Negtol, and the Distribution columns are used to
specify the tolerance information. In the Postol and Negtol
columns, specify the positive and negative tolerances,
respectively, for each of the simulation parameters. Adding a
tolerance value enables the Distribution field for the
parameter. The possible distribution types are:
■
172
FLAT - Use the flat distribution function if you want an
equal probability of one parameter value being chosen
over another.
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
■
BSIMD.4.2 - Use the bimodal distribution function if you
want to represent the probability of a manufactured
component falling in the outer range of tolerance values.
■
GAUSS0.4 - Use the Gaussian distribution function if you
want a bell curve probability that one parameter value will
be chosen versus another.
■
SKEW.4.8 - Use the skewed distribution function if you
want to weigh the probability of one parameter value
being chosen versus another.
By default, the distribution type is FLAT. The distribution type
influences the Sensitivity and Monte Carlo analysis. To know
more about Sensitivity and Monte Carlo analysis, see PSpice
Advanced Analysis User’s Guide.
To find out more about the distribution functions, see the
technical note, Specifying Advanced Analysis Monte
Carlo Distribution Functions at www.orcadpcb.com.
Model Editor-supported device types based on PSpice templates
Table 4-3 lists the device types for which template-based
models can be created using the Model Editor.
Table 4-3 Template-based device types supported in
Model Editor
This part
PSpice User's Guide
type1...
And this name
prefix2...
diode3
X
bipolar transistor
X
IGBT
X
JFET
X
Power MOSFET
X
operational amplifier
X
voltage regulator
X
magnetic core4
K
173
Chapter 4
Creating and editing models
Product Version 10.5
1. For template-based PSpice models the model text is
read-only and cannot be edited using the Model Editor.
2. This is the standard PSpice device letter notation. Refer to the
online PSpice Reference Guide.
3. The part type DIODE is the only part supported in PSpice A/D
Basics.
4. A template-based magnetic core model is a SpicePlus model.
To find out more about Magnetic Core models, see PSpice
Reference Manual.
Importing an existing model
You can import third-party or vendor-provided Spice models
into a format understood by the Model Editor. Importing a
model enables editing the model using the Model Editor user
interface.
1
Open the Model Editor.
From the Start menu, point to Release OrCAD 10.0 in the
Programs folder, choose PSpice Accessories and then
choose Model Editor.
2
Open a model library.
From the File menu, choose New or Open.
3
From the Model menu, choose Import.
4
Select the file containing the model definition and select
Open.
The imported model appears in the model library.
Although, only the first model of the selected library file is
imported to the Model Editor, it is recommended that the
file selected in step 4 should contain only one model
definition.
Caution
The device property file associated with the
model is not imported.
174
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
Enabling and disabling automatic part creation
Part creation in the Model Editor is optional. By default,
automatic part creation is enabled. However, if you previously
disabled part creation, you will need to enable it before
creating a new model and part.
Instead of using the PSpice default part set for new models,
you can have the Model Editor use your own set of standard
parts. To find out more, see Basing new parts on a custom set
of parts on page 254.
To automatically create parts for new models
1
From the Tools menu, choose Options.
2
Select the Always Create Part when Saving Model option
if it is not already checked.
3
Under Schematic Editor, select Capture.
4
Under Save Part To, enter the name of the part library for
the new part. Choose either:
❑
Part Library Path Same As Model Library to create or
open the *.OLB file that has the same name prefix
as the currently open model library (*.LIB).
Example: If the model library is MYPARTS.LIB, then
the Model Editor creates the part library
MYPARTS.OLB.
❑
User-Defined Part Library, and then enter a file name
in the Part Library Name text box.
Note: If you select a user-defined Part library, the Model
Editor saves all new parts to the specified file until you
change it.
Saving global models (and parts)
When you save your changes, the Model Editor does the
following for you:
PSpice User's Guide
175
Chapter 4
Creating and editing models
Product Version 10.5
■
Saves the model definition to the model library that you
originally opened.
■
If you had the automatic part creation option enabled,
saves the part definition to
MODEL_LIBRARY_NAME.OLB.
If you want to save the open model library to a new library,
then:
1
From the File menu, choose Save As.
2
Enter the name of the new model library.
If you want to save only the model definition that you are
currently editing to a different library, then
1
From the Model menu, select Export.
2
Enter the name of the new file.
Note: When you use the Export command, the model
definition is saved with a .MOD extension.
3
If you want PSpice to search this file automatically,
configure it in Capture (using the Library files list in the
Configuration Files tab on the Simulation Settings dialog
box).
You cannot export multiple models to a single MOD file.
Exporting a model to the same file overwrites the original
contents of the MOD file.
To save the new model (and part)
1
From the File menu, choose Save to update
MODEL_LIBRARY_NAME.LIB,
MODEL_LIBRARY_NAME.PRP (and, if you enabled part
creation, MODEL_LIBRARY_NAME directory), and save
them to disk.
Note: To simulate the model, add the Model Library (.LIB) to
the project using the PSpice menu, Edit Profile,
Simulation Settings dialog box. Click the Configuration
Files tab, click Library in the Category field, browse to
the Model Library, and click the Add to Design button.
176
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
Running the Model Editor from the schematic editor
Start the Model Editor from the schematic editor when you
want to:
■
define tolerances on model parameters for statistical
analysis (see Example: editing a Q2N2222 instance
model on page 195)
■
test behavior variations on a part, or
■
refine a model before making it available to all designs.
This means editing models for part instances on your
schematic page. When you select a part instance and edit its
model, the Model Editor automatically creates an instance
model that you can then change.
Once you have started the Model Editor, you can proceed with
entering data sheet information and model fitting as described
in How to fit models on page 169.
You can also use the Model Editor to view the syntax for a
model definition. When you have finished viewing, be sure to
quit the Model Editor without saving the library, so that the
schematic page editor does not create an instance model.
Note: When the Model Editor is invoked from a schematic
editor, the part creation feature is disabled.
What is an instance model?
An instance model is a copy of the part’s original model. The
copied model is local to the design. You can customize the
instance model without impacting any other design that uses
the original part from the library.
Instance models are created only when you want to edit
models from global libraries. If you open a model for editing
from a local library, after editing, the model will be saved in the
same local library. For more information on global and local
libraries see Global vs. design vs. profile models and libraries on
page 153.
PSpice User's Guide
177
Chapter 4
Creating and editing models
Product Version 10.5
When the schematic editor creates the copy, it saves a copy of
the model in DESIGN_NAME.LIB.
For more information on instance models, see Reusing
instance models on page 200.
Starting the Model Editor
To start editing an instance model
1
In Capture, select one part on your schematic page.
2
From the Edit menu, choose PSpice Model.
The schematic page editor searches the model libraries
for the instance model. To find out how Capture searches
the library, see Changing model library search order on
page 208.
❑
If found, the schematic page editor starts the Model
Editor, which opens the design library and loads the
instance model.
❑
If not found, the schematic page editor assumes that
this is a new instance model and does the following:
makes a copy of the original model definition in the
DESIGN_NAME.LIB and starts the Model Editor
with the new model loaded.
After you start the Model Editor, you can proceed to
change the text as described in To display the model text
on page 193.
Saving design models
When you save your edits, the following is done for you to
make sure the instance model is linked to the selected part
instances in your design:
178
■
The Model Editor saves the model definition to
DESIGN_NAME.LIB.
■
If the library is new, the Model Editor configures
DESIGN_NAME.LIB for local use.
PSpice User's Guide
Product Version 10.5
Creating models using the Model Editor
The schematic page editor assigns the new model name to
the Implementation property for each of the selected part
instances (see What happens if you don’t save the instance
model on page 179).
Actions that automatically configure the instance model
library for global use
Instance model libraries are normally configured for design
use. However, if you perform the following action, the Model
Editor configures the library for global use instead:
■
Save the model to a different library by typing a new file
name in the Library text box in the Save To frame.
To save instance models
1
From the File menu, choose Save to update
DESIGN_NAME.LIB and save it to disk.
What happens if you don’t save the instance model
Before the schematic page editor starts the Model Editor, it
does the following:
■
Makes a copy of the original model and saves it as an
instance model in SCHEMATIC_NAME.LIB.
■
Configures SCHEMATIC_NAME.LIB for design use, if
not already done.
■
Attaches the new instance model name to the
Implementation property for the selected part instance.
This means that if you:
■
quit the Model Editor, or
■
return to Capture to simulate the design
without first saving the model you are editing, the part
instance on your schematic page is still attached to the
instance model implementation.
PSpice User's Guide
179
Chapter 4
Creating and editing models
Product Version 10.5
In this case, the instance model is identical to the original
model. If you decide to edit this model later, be sure to do one
of the following:
■
If you want the changes to remain specific to the current
design, edit the instance model in the design library using
the Model Editor.
■
If you want the change to be global, change the model
implementation for the part instance in your design back
to the original model name in the global library, and then
edit the original model from within the part editor.
To find out how to change model references, see Changing
the model reference to an existing model definition on
page 199.
Model creation examples
Examples covered in this section cover how to use the Model
Editor to create simulation models based on:
■
Device characteristic curves. See Example: Creating a
PSpice model based on device characteristic curves.
■
PSpice-provided templates. See Example: Creating
template-based PSpice model on page 187.
Example: Creating a PSpice model based on device characteristic curves
In this example, you will model a simple diode device as
follows:
180
■
Create the schematic for a simple half-wave rectifier.
■
Create a new model for a diode.
■
Attach new model to the D1 diode.
PSpice User's Guide
Product Version 10.5
Model creation examples
Creating the half-wave rectifier design
Figure 4-4 Design for a
half-wave rectifier.
To draw the design
1
From the Project Manager, from the File menu point to
New, then choose Project.
2
In the New Project dialog box, ensure that the Analog or
Mixed A/D option is selected.
3
Enter the name of the new project (RECTFR) and click
Create.
4
From the Capture Place menu, choose Part.
5
Place one each of the following parts (reference
designator shown in parentheses) as shown in
Figure 4-4:
❑
Dbreak (D1 diode)
❑
C (C1 capacitor)
❑
R (R1 resistor)
❑
VSIN (V1 sine wave source)
6
Click the Ground button
on the tool palette and place
the ‘0’ analog ground from the SOURCE.OLB part library.
7
From the Place menu, choose Wire, and draw the
connections between parts as shown in Figure 4-4.
8
From the File menu, choose Save.
Note: If you were to simulate this design using a transient
analysis, you would also need to set up a transient
PSpice User's Guide
181
Chapter 4
Creating and editing models
Product Version 10.5
specification for V1; most likely, this would mean
defining the VOFF (offset voltage), VAMPL (amplitude),
and FREQ (frequency) properties for V1. For this
tutorial, however, you will not perform a simulation, so
you can skip this step.
Using the Model Editor to edit the D1 diode model
To create a new model and model library
1
Open the Model Editor.
2
From the File menu in the Model Editor, choose New.
3
From the Model menu, choose New.
4
In the New dialog box, do the following:
a. In the Model Name text box, type DbreakX.
b. Select Use Device Characteristic Curves.
c. From the From Model list, select Diode.
d. Click OK.
5
From the File menu, choose Save.
By default, the updated model is saved in the
RECTFR.LIB library.
Entering data sheet information
As shown in Figure 4-5, the Model Editor initially displays:
■
182
diode model characteristics listed in the Models List
window, and
PSpice User's Guide
Product Version 10.5
Model creation examples
■
DbreakX model parameter values listed in the
Parameters window.
Figure 4-5 Model characteristics and parameter values
for DbreakX.
You can modify each model characteristic shown in the Model
Spec frame with new values from data sheets. The Model
Editor takes the new information and fits new model
parameter values.
When updating the entered data, the Model Editor expects
either:
■
device curve data (point pairs) or
■
single-valued data
depending on the device characteristic.
For the diode, Forward Current, Junction Capacitance, and
Reverse Leakage require device curve data. Reverse
Breakdown and Reverse Recovery require single-valued data.
PSpice User's Guide
183
Chapter 4
Creating and editing models
Product Version 10.5
Table 4-4 lists the data sheet information for the DbreakX
model.
Table 4-4 Sample diode data sheet values
For this model
characteristic...
Enter this...
forward current
(1.3, 0.2)
junction capacitance
(1m, 120p) (1, 73p) (3.75, 45p)
reverse leakage
(6, 20n)
reverse breakdown
(Vz=7.5, Iz=20m, Zz=5)
reverse recovery
no changes
To change the Forward Current characteristic
1
In the Spec Entry frame, click the Forward Current tab.
This tab requires curve data.
2
In the Vfwd text box, type 1.3.
3
Press Tab to move to the Ifwd text box, and then type
0.2.
To change the values for Junction Capacitance and
Reverse Leakage
Follow the same steps as for Forward Current, entering the
data sheet information listed in Table 4-4 that corresponds to
the current model characteristic.
To change the Reverse Breakdown characteristic
1
In the Spec Editing frame, click the Reverse Breakdown
tab.
This tab requires single-valued data.
2
In the Vz text box, type 7.5.
Note: The Model Editor accepts the same scale factors
184
PSpice User's Guide
Product Version 10.5
Model creation examples
normally accepted by PSpice.
3
Press Tab to move to the Iz text box, and then type 20m.
4
Press Tab to move to the Zz text box, and then type 5.
Extracting model parameters
To generate new model parameter values
1
From the Tools menu, choose Extract Parameters.
A check mark appears in the Active column of the
Parameters frame for each extracted model parameter.
To display the curves for the five diode characteristics
1
From the Window menu, choose Tile.
Some of the plots are shown in Figure 4-6 below.
Figure 4-6 Assorted device characteristic curves for a
diode.
You can also do the following with an active plot window:
■
PSpice User's Guide
Pan and zoom within the plot using commands on the
View menu.
185
Chapter 4
Creating and editing models
■
Product Version 10.5
Rescale axes using the Axis Settings command on the
Plot menu.
Adding curves for more than one temperature
By default, the Model Editor computes device curves at 27°C.
For any characteristic, you can add curves to the plot at other
temperatures.
To add curves for Forward Current at a different
temperature
1
In the Spec Entry frame, click the Forward Current tab.
2
From the Plot menu, choose Add Trace.
3
Type 100 (in °C).
4
Click OK.
The Forward Current plot should appear as shown in
Figure 4-7.
Figure 4-7 Forward Current device curve at two
temperatures.
Completing the model definition
You can refine the model definition by:
■
186
modifying the entered data as described before, or
PSpice User's Guide
Product Version 10.5
Model creation examples
■
editing model parameters directly.
You can update individual model parameters by editing them
in the Parameters frame of the Model Editor workspace. When
you save the model library, the Model Editor automatically
updates the device curves.
For this tutorial, leave the model parameters at their current
settings.
To save the model definition with the current parameter
values and to make the model available to your design
1
From the File menu, select Save to update RECTFR.LIB
and save the library to disk.
The model definition is now complete. You can use this
model definition in your design.
Attaching the DbreakX model to the D1 diode
1
In Capture, open the RECTFR project.
2
Select the D1 diode.
3
From the Edit menu, choose Properties.
4
In the Property Editor dialog box, change the value of
Implementation property from Dbreak to DbreakX.
To know more about the Implementation property, see
MODEL on page 260.
5
Close the dialog box, and save the design.
Your design is ready to simulate with the model definition
you just created.
Example: Creating template-based PSpice model
In this example, you will create a template-based PSpice
model for an operational amplifier, using the Model Editor.
The template-based OPAMP model is the only model created
using the Model Editor that has multiple level support for
PSpice User's Guide
187
Chapter 4
Creating and editing models
Product Version 10.5
simulation parameters. Tasks that will be covered in this
example are:
■
Creating a new template-based PSpice model for
Operational Amplifier
■
Multiple level support for template-based OPAMP models
in the Model Editor
Multiple level support implies that the number of
simulation parameters used in the model varies with the
model level. The higher the level, the more are the
number of simulation parameters.
The models with a higher number of simulation
parameters are closer to the real life devices. Therefore,
the simulation results are more accurate when high level
models are used. Use lower level simulation models to
minimize the simulation time.
Creating a new model
188
1
Start the Model Editor alone.
2
From the File menu, choose New to create a new library.
3
From the Model menu, choose New.
4
In the New dialog box, specify the name of the new model
as OPA_LOCAL.
5
Select the Use Templates option.
6
To specify the device type, select Operational Amplifier
from the From Model drop-down list.
PSpice User's Guide
Product Version 10.5
Model creation examples
7
Specify the type of OPAMP to be created. In this example,
select options to create an internally compensated
bipolar operational amplifier with PNP input.
Figure 4-8 The New dialog box
8
Click OK.
The Simulation Parameters and the Model Text windows
appear. In the Models List, three models, OPA_LOCAL_1,
OPA_LOCAL_2, and OPA_LOCAL_3 appear.
Caution
The Model Editor creates multiple models only for
Advanced Analysis OPAMP models. This is
because, template-based OPAMP models
support multiple levels of simulation parameters,
and the Model Editor creates one model for each
level.
The OPA_LOCAL_3 model contains all the simulation
parameters available in the OPA_LOCAL_2 model plus
some extra simulation parameters. The OPA_LOCAL_2
PSpice User's Guide
189
Chapter 4
Creating and editing models
Product Version 10.5
model contains some additional simulation parameters
besides the ones listed in the OPA_LOCAL_1 model.
9
Select the OPA_LOCAL_3 model, and edit the values of
the simulation parameters listed in Table 4-5. Table 4-5
lists the simulation parameters along with the new values.
For other simulation parameters not listed in the table,
accept the default values.
Table 4-5 List of Simulation Parameters to be modified
Simulation
Property
Name
Value
Distribu Postive
tion
Tolerance
(Postol)
Negative
Tolerance
(Negtol)
VOS
1e-7
FLAT
10%
10%
IB
default
FLAT
10%
10%
IBOS
default
FLAT
10%
10%
A0
1000000
FLAT
10%
10%
GBW
default
FLAT
10%
10%
SRP
1.0e+6
FLAT
10%
10%
SRM
1.0e+6
FLAT
10%
10%
CMRR
default
FLAT
10%
10%
10 To ensure that the values entered by you in the Simulation
Parameters frame overwrite the default value of the
simulation parameters, check the Editable check box for
all the simulation properties.
Selecting the Editable check box ensures that the
simulation parameter value:
190
❑
entered by users will overwrite the values in the
template property file.
❑
appears in the device property file.
❑
can be directly passed from the schematic editor as
properties attached to the symbol.
PSpice User's Guide
Product Version 10.5
Model creation examples
In such cases, the values of the simulation parameters
can be picked up from following three locations in the
decreasing order of priority:
❑
schematic editor
❑
device property file
❑
template property file
11 After making the simulation parameters editable, save the
model. Specify the library name as LOCAL_LIB.
All the changes in the OPA_LOCAL_3 model are reflected
in the OPA_LOCAL_2 and OPA_LOCAL_1 models also.
This is because all three models have a common section
for the simulation and smoke parameters in the device
property file, LOCAL_LIB.PRP.
Caution
It is recommended that multiple level models
created using the Model Editor should be used
cautiously especially when used in different
designs.
Consider a situation where you use OPA_LOCAL_1 from
the LOCAL_LIB library in design A and OPA_LOCAL_3
from the LOCAL_LIB library in design B. Any changes
that you make to the simulation or smoke parameter
values of the OPA_LOCAL_1 model for design A will also
be reflected in the OPA_LOCAL_3 model used in design
B.
After you have saved your changes in the Model Editor, the
following files are generated:
■
LOCAL_LIB.LIB - The library file containing model
information.
■
LOCAL_LIB.PRP - The device property file containing
device specific information for all the models in the
LOCAL_LIB.LIB.
Saving the LOCAL_LIB library completes the tasks of creating
a template-based PSpice model for Operational Amplifier.
PSpice User's Guide
191
Chapter 4
Creating and editing models
Product Version 10.5
Because of the multiple-level support for Advanced Analysis
OPAMP models in the Model Editor, instead of one, three
models are created.
Note: Deleting a Model Editor-created multiple-level model
deletes the model only from the library. The model
information is not deleted from the device property file.
This is because, all three OPAMP models are linked to
the same section in the device property file. The device
property section for the model will be deleted only after
all the linked models are deleted.
Note: If you have Advanced Analysis installed, the Smoke tab
also appears besides the Simulation tab, and you can
also add smoke information to the model. See Adding
smoke information to the OPA_LOCAL operational
amplifier model on page 216.
Note: Example covered in the section, Creating parts in the
batch mode on page 246 in Chapter 5, “Creating parts
for models” is an extension of this example. It covers
part creation using Model Editor and using Model
Editor-created parts in a schematic.
192
PSpice User's Guide
Product Version 10.5
Model creation examples
Editing model text
Note: This section is valid only for PSpice models that are
based on device characteristic curves.
The Model Text is editable only for PSpice models. For
template-based PSpice models, the Model Text window is
read-only.
Caution
If you edit the text of a model that was created by
entering data sheet values, you may not be able
to edit the model in the Extract Model view again.
For any model, you can edit model text in the Model Editor
instead of using the Spec Entry and Parameter frames.
However, there are two cases where you must edit the model
text:
■
When you want to edit models of device types not
supported by the Model Editor. The model text is
displayed automatically when you load one of these
models.
■
When you want to add DEV and LOT tolerances for
Monte Carlo or sensitivity/worst-case analysis.
By typing PSpice commands and netlist entries, you can do
the following:
■
change definitions, and
■
create new definitions
When you have finished, the Model Editor automatically
configures the model definitions into the model libraries.
To display the model text
1
From the View menu, choose Edit Model.
The Model Editor displays the PSpice syntax for model
definitions:
PSpice User's Guide
193
Chapter 4
Creating and editing models
Product Version 10.5
❑
.MODEL syntax for models defined as parameter
sets
❑
.SUBCKT syntax for models defined as netlist
subcircuits
You can edit the definition just as you would in any
standard text editor.
To find out more about PSpice command and netlist syntax,
refer to the online PSpice Reference Guide.
Editing .MODEL definitions
For definitions implemented as model parameter sets using
the PSpice .MODEL syntax, the Model Editor lists one
parameter per line. This makes it easier to add DEV/LOT
tolerances to model parameters for Monte Carlo or
sensitivity/worst-case analysis.
Editing .SUBCKT definitions
For definitions implemented as subcircuit netlists using the
PSpice .SUBCKT syntax, the Model Editor displays the
subcircuit syntax exactly as it appears in the model library. The
Model Editor also includes all of the comments immediately
before or after the subcircuit definition.
Changing the model name
You can change the model name directly in the PSpice
.MODEL or .SUBCKT syntax, but double-check that the new
name does not conflict with models already contained in the
libraries. To find out more about instance model naming
conventions, see What is an instance model? on page 177.
Note: If you do create a model with the same name as
another model and want PSpice to always use your
model, make sure the configured model libraries are
ordered such that your definition precedes any other
definitions. To find out more about search order in the
model library, see Changing model library search order
on page 208.
194
PSpice User's Guide
Product Version 10.5
Model creation examples
Example: editing a Q2N2222 instance model
Suppose you have a design named MY.OPJ that contains
several instances of a Q2N2222 bipolar transistor. If you want
to see the effect of base resistance variation on one specific
device, Q6, you need to do the following:
■
Define a tolerance (in this example, 5%) on the Rb model
parameter.
Important
Adding tolerance to a device characteristic
curve-based model does not make it compatible for
use with Advanced Analysis Monte Carlo.
■
Set up and run PSpice Monte Carlo analysis.
The following example demonstrates how to set up the
instance model for Q6.
Starting the Model Editor
To start the Model Editor,
1
In the schematic page editor, select Q6 on the schematic
page.
2
From the Edit menu, choose PSpice Model.
The Model Editor automatically creates a copy of the
Q2N2222 base model definition.
3
In the Model Editor, from the View menu, choose Model
Text.
The Model Editor displays the PSpice syntax for the
copied model in the text editing area.
Editing the Q2N2222 model instance
Text edits appropriate to this example are as follows:
■
PSpice User's Guide
Add the DEV 5% clause to the Rb statement (required).
195
Chapter 4
Creating and editing models
■
Product Version 10.5
Change the model name to Q2N2222-MC (optional, for
descriptive purposes only).
To find out more about PSpice command and netlist syntax,
refer to the online PSpice Reference Guide.
Saving the edits and updating the schematic
When you choose Save from the File menu, two things
happen:
■
The Model Editor saves the model definition to the model
library.
■
The schematic page editor updates the Implementation
property value to Q2N2222-MC for the Q6 part instance.
In this example, the default model library is MY.LIB. If
MY.LIB does not already exist, the Model Editor creates and
saves it in the current working directory. The schematic page
editor then automatically configures it as a design model
library for use with the current design only.
Now you are ready to set up and run the Monte Carlo analysis.
Note: If you verify the model library configuration (in the
Simulation Settings dialog box, click the Configuration
Files tab and view the Library files list), you see entries
for
NOM.LIB (for global use, as denoted by the
icon) and
MY.LIB (for design use, as denoted by the
icon) in the Library files list.
You can change the model reference for this part back
to the original Q2N2222 by following the procedure To
change model references for part instances on your
design on page 199.
Using the Create Subcircuit Format Netlist command
The Create Subcircuit Format Netlist command is used from
Capture. This command creates a subcircuit netlist definition
for the displayed level of hierarchy and all lower levels in your
design.
196
PSpice User's Guide
Product Version 10.5
Using the Create Subcircuit Format Netlist command
Note: The Create Subcircuit Format Netlist command does
not help you create a hierarchical design. You need to
do this yourself before using the Create Subcircuit
Format Netlist command. For information on
hierarchical designs and how to create them, refer to
the OrCAD Capture User’s Guide.
The schematic page editor does the following things for you:
■
Maps any named interface ports at the active level of
hierarchy to terminal nodes in the PSpice .SUBCKT
statement.
■
Saves the subcircuit definition to a file named
DESIGN_NAME-SCHEMATIC_NAME.LIB.
Before you can use the subcircuit definition in your design, you
need to:
■
Create a part for the subcircuit.
■
Configure the
DESIGN_NAME-SCHEMATIC_NAME.LIB file so
PSpice knows where to find it.
To create a subcircuit definition for a portion of your
design
To create a subcircuit netlist definition
PSpice User's Guide
1
In the Project Manager, select the schematic folder that
contains the circuitry for which a subcircuit netlist
definition is to be created.
2
If the schematic folder is not the root folder, choose Make
Root from the Design menu. You may be prompted to
save the design first.
3
In the Project Manager, from the Tools menu, choose
Create Netlist.
4
Select the PSpice tab.
5
In the Options frame, select Create SubCircuit Format
Netlist.
197
Chapter 4
Creating and editing models
6
Product Version 10.5
Click OK to generate the subcircuit definition and save it
to DESIGN_NAME-SCHEMATIC_NAME.LIB.
To create a part for the subcircuit netlist definition
1
Open the Model Editor alone.
2
From the File menu, select the Open command and open
the DESIGN_NAME-SCHEMATIC_NAME.LIB file.
3
Select the model from the Models List and, if necessary,
refine the subcircuit definition.
Refinements can include extending the subcircuit
definition using the optional nodes construct,
OPTIONAL:, the variable parameters construct,
PARAMS:, and the .FUNC and local .PARAM commands.
4
From the File menu, select Create Capture Parts.
5
In the Enter Input Model Library text box, browse and
open the DESIGN_NAME-SCHEMATIC_NAME.LIB file.
Note: The Enter Output Part Library is automatically
filled in with the
DESIGN_NAME-SCHEMATIC_NAME.OLB file.
6
Click OK and OK again to clear the .ERR log window.
The subcircuit part is now ready for use in a design.
To configure the subcircuit file
198
1
In the schematic page editor, from the PSpice menu,
choose Edit Profile to display the Simulation Settings
dialog box.
2
Click the Configuration Files tab.
3
Click either Library or Include in the Category field of the
Configuration Files tab, and then configure
DESIGN_NAME-SCHEMATIC_NAME.LIB as either a
model library or an include file (see Configuring model
libraries on page 202).
PSpice User's Guide
Product Version 10.5
Changing the model reference to an existing model definition
Changing the model reference to an existing model
definition
Parts are linked to models by the model name assigned to the
parts’ Implementation property. You can change this
assignment by replacing the Implementation property value
with the name of a different model that already exists in the
library.
You can do this for:
■
A part instance in your design.
■
A part in the part library.
To change model references for part instances on your
design
1
Find the name of the model that you want to use.
2
In the schematic page editor, select one or more parts on
your schematic page.
3
From the Edit menu, choose Properties.
The Parts spreadsheet appears.
4
Click the cell under the column Implementation Type.
5
From the Implementation list, select PSpice Model.
6
In the Implementation column, type the name of the
existing model that you want to use if it is not already
listed.
7
Click Apply to update the changes, then close the
spreadsheet.
To change the model reference for a part in the part
library
PSpice User's Guide
1
Find the name of the model that you want to use.
2
In the schematic page editor, select the part you want to
change.
199
Chapter 4
Creating and editing models
Product Version 10.5
3
From the Edit menu, choose Part to load the part in the
part editor for editing.
4
From the Options menu, choose Part Properties to
display the User Properties dialog box.
5
Select Implementation Type.
6
From the Implementation list, select PSpice Model.
7
In the Implementation text box, type the name of the
existing model that you want to use if it is not already
listed.
8
Click OK to close the Edit Part dialog box.
Reusing instance models
If you created instance models in your design and want to
reuse them, there are two things you can do:
■
Attach the instance model implementation to other part
instances in the same design.
■
Change the instance model to a global model and create
a part that corresponds to it.
For information on how to create instance models, see:
■
Running the Model Editor from the schematic editor on
page 177.
■
Starting the Model Editor on page 178.
Reusing instance models in the same schematic
There are two ways to use the instance model elsewhere in
the same design.
To use the instance model elsewhere in your design
Do one of the following:
■
200
Change the model reference for other part instances to
the name of the new model instance.
PSpice User's Guide
Product Version 10.5
Reusing instance models
See Changing the model reference to an existing model
definition on page 199.
■
From the Edit menu, use the Copy and Paste commands
to place more part instances.
Making instance models available to all designs
If you are refining model behavior specific to your design, and
are ready to make it available to any design, then you need to
link the model definition to a part and configure it for global
use.
To make your instance model available to any design
1
Create a part and assign the instance model name to the
Implementation property. See Chapter 5, “Creating parts for
models” for more information.
2
If needed, move the instance model definition to an
appropriate model library, and make sure the library is
configured for global use. See Configuring model libraries
on page 202 for more information.
Note: If you use the part wizard to create the part
automatically from the model definition, then this step
is completed for you.
PSpice User's Guide
201
Chapter 4
Creating and editing models
Product Version 10.5
Configuring model libraries
Although model libraries are usually configured for you, there
are things that you sometimes must do yourself. These are:
■
adding new model libraries that were created outside of
Capture or the Model Editor
■
changing the global, design or profile scope of a model
library
■
changing the library search order
■
changing or adding directory search paths
The Configuration Files tab
The Configuration Files tab of the Simulation Settings dialog
box lets you add, change, and remove model libraries and
include files from the configuration or modify the search order.
Note: Removing a library in this dialog box means that you
are removing the model library from the configured list.
The library still exists on your computer and you can
add it back to the configuration later.
To display the Library files list
202
1
In PSpice, open or create a PSpice project.
2
From the PSpice menu, choose either New Simulation
Profile or Edit Profile if a profile already exists.
3
Click the Configuration Files tab in the Simulation
Settings dialog box.
PSpice User's Guide
Product Version 10.5
Reusing instance models
4
Click Library in the Category field to display the Library
files list.
The Library files list shows the model libraries that PSpice
searches for definitions matching the parts in your
design. Files showing an
icon after their name have
global scope; files having the
icon have a design
scope and files with the
icon have a profile scope.
The buttons for adding model libraries to the configuration
follow the same profile/local/global syntax convention.
Click one of the following:
❑
Add to Profile for profile models
❑
Add to Design for design models.
❑
Add as Global for global models.
The Include files list in the Configuration Files tab contains
include files. You can manually add profile, design and global
include files to your configuration using the Add to Profile, Add
to Design and Add as Global buttons, respectively.
The Stimulus files list in the Configuration Files tab contains
stimulus files. See Configuring stimulus files on page 477 for
more information.
How PSpice uses model libraries
PSpice searches libraries for any information it needs to
complete the definition of a part or to run a simulation. If an
up-to-date index does not already exist, PSpice automatically
generates an index file and uses the index to access only the
model definitions relevant to the simulation. This means:
PSpice User's Guide
■
Disk space is not used up with definitions that your design
does not use.
■
There is no memory penalty for having large model
libraries.
■
Loading time is kept to a minimum.
203
Chapter 4
Creating and editing models
Product Version 10.5
Caution—When you use include files instead
PSpice treats model library and include files differently as
follows:
■
For model library files, PSpice reads in only the
definitions it needs to run the current simulation.
■
For include files, PSpice reads in the file in its entirety.
This implies that if you configure a model library (*.LIB
extension) as an include file using the Add to Design or Add
as Global button, PSpice loads every model definition
contained in that file.
If the model library is large, you might overload the memory
capacity of your system. However, when developing models,
you can do the following:
1
Initially configure the model library as an include file; this
avoids rebuilding the index files every time the model
library changes.
2
When your models are stable, reconfigure the include file
containing the model definitions as a library file.
To reconfigure an include file as a model library file:
1
From the Simulation menu, choose Edit Profile, then click
the Configuration Files tab.
2
Click Include in the Category field to display the Include
files list.
3
Select the include file that you want to change.
4
Click the Delete button located above the Include files list.
See Adding model libraries to the configuration on page 205.
Search order
When searching for model definitions, PSpice scans the
model libraries using these criteria:
■
204
profile model libraries before design model libraries
PSpice User's Guide
Product Version 10.5
Reusing instance models
■
design model libraries before global model libraries
■
model library sequence as listed in the Library files list in
the Configuration Files tab of the Simulation Settings
dialog box
■
list of directories (including the design library) specified in
the library search path in the order given (see Changing
the library search path on page 210). From the directories
listed in the Library Path, only the directories that contain
a NOM.LIB file are looked up by PSpice during the model
search.
Tip
The search order for the device property files is same
as that of the model library files. The .PRP files are
searched along with the .LIB files.
Handling duplicate model names
If two or more model libraries contain models with the same
name, PSpice always uses the first model it finds. This means
you might need to modify the search order to make sure
PSpice uses the model that you want. See Changing model
library search order on page 208.
Note: PSpice searches profile libraries before design
libraries and design libraries before global libraries.
Therefore, if the new model you want to use is specific
to your profile and the duplicate definition is design or
global, you do not need to make any changes.
Similarly, if the new model you want to use is specific to
your design and the duplicate definition is global, you
do not need to make any changes.
Adding model libraries to the configuration
New libraries are added above the selected library name in
the Library files list box.
PSpice User's Guide
205
Chapter 4
Creating and editing models
Product Version 10.5
To add model libraries to the configuration
1
From the Simulation menu, choose Edit Profile, then click
the Configuration Files tab.
2
Click Library in the Category field to display the Library
files list.
3
Click the library name positioned one entry below where
you want to add the new library.
4
In the Filename text box, either:
5
6
❑
type the name of the model library, or
❑
click Browse to locate and select the library.
Do one of the following:
❑
If the model definitions are for use in the current
profile only, click the Add to Profile button.
❑
If the model definitions are for use in the current
design only, click the Add to Design button.
❑
If the model definitions are for global use in any
schematic, click the Add as Global button instead.
Click OK.
Note: If the model libraries reside in a directory that is not on
the library search path, and you use the Browse button
in step 4 to select the libraries you want to add, then the
schematic editor automatically updates the library
search path to include the selected library in the search
path. Otherwise, you need to add the directory path
yourself. See Changing the library search path on
page 210.
Changing the model library scope from profile to design, profile to global,
design to global and vice versa
There are times when you might need to change the scope of
a model library from profile to design, profile to global, design
to global, or vice versa.
206
PSpice User's Guide
Product Version 10.5
Reusing instance models
Example: If you have an instance model that you now want to
make available to any design, then you need to set the scope
of the local model library that contains it to global.
For more information, see Global vs. design vs. profile models
and libraries on page 153.
To change the scope of a design model to global
1
From the Simulation menu, choose Edit Profile, then click
the Configuration Files tab.
2
Click Library in the Category field to display the Library
files list.
3
Select the model library that you want to change.
4
Click the Delete toolbar button to remove the local entry.
5
Add the model library as a global entry.
For more information, see Adding model libraries to the
configuration on page 205.
PSpice User's Guide
207
Chapter 4
Creating and editing models
Product Version 10.5
Changing model library search order
Two reasons why you might want to change the search order
are to:
■
reduce the search time
■
avoid using the wrong model when there are model
names duplicated across libraries. PSpice A/D always
uses the first instance. See Handling duplicate model names
on page 205 for more information.
To change the order of libraries
1
Click the Configuration Files tab in the Simulation
Settings dialog box.
2
Click Library in the Category field to display the Library
files list. On the Library files list of the Configuration Files
tab:
a. Select the library name you wish to move.
b. Use either the Up Arrow or Down Arrow toolbar
button to move the library name to a different place
in the list.
Note: You can only change the order of libraries that
have the same scope. This implies that though you can
change the order of profile libraries, local libraries and
global libraries, you cannot place a global library before a
local library or a local library before a profile library.
3
If you have listed multiple *.LIB commands within a
single library (like NOM.LIB), then edit the library using a
text editor to change the order.
Example: The model libraries DIODES.LIB and
EDIODES.LIB (European manufactured diodes) shipped
with your PSpice programs have identically named device
definitions. If your design uses a device out of one of
these libraries, you need to position the model library
containing the definition of choice earlier in the list. If your
system is configured as originally shipped, this means
you need to add the specific library to the list before
NOM.LIB.
208
PSpice User's Guide
Product Version 10.5
Reusing instance models
Caution
Do not edit NOM.LIB. If you do, PSpice will
recreate the indexes for every model library
referenced in NOM.LIB. This can take some time.
4
PSpice User's Guide
After you have modified the library settings using the
Simulation Settings dialog box, you must first select the
design name in the Project Manager and then save the
design by clicking the save button. This must be done
every time you make a change in the Simulation Settings
dialog box. This is to ensure that the changes in the
simulation settings are reflected in the .OPJ file and are
picked up the netlister in the subsequent flows.
209
Chapter 4
Creating and editing models
Product Version 10.5
Changing the library search path
For model libraries that are configured without explicit path
names, PSpice first searches the directory where the current
design resides, then steps down the list of directories
specified in the Library Path text box on the Library files list in
the Configuration Files tab of the Simulation Settings dialog
box.
To change the library search path
210
1
From the Simulation menu, choose Edit Profile to display
the Simulation Settings dialog box.
2
Click the Configuration Files tab.
3
Click Library in the Category field to display the Library
files list.
4
In the Library Path text box, position the pointer after the
directory path that PSpice should search before the new
path.
5
Type in the new path name following these rules:
❑
Use a semicolon character ( ; ) to separate two path
names.
❑
Do not follow the last path name with a semicolon.
PSpice User's Guide
Product Version 10.5
Reusing instance models
Example: To search first C:\ORCAD\PSPICE\
LIBRARY, then C:\MYLIBS, for model libraries, type
"C:\ORCAD\PSPICE\LIBRARY";
"C:\MYLIBS"
in the Library Path text box.
PSpice User's Guide
211
Chapter 4
Creating and editing models
Product Version 10.5
Handling smoke information using the Model Editor
You can use the Model Editor to add smoke information to a
device type supported by the Model Editor. This feature is
available only if you have PSpice Advanced Analysis installed.
Using the Model Editor, you can:
■
Add smoke information PSpice models.
■
Create template-base PSpice models with smoke
information.
■
Edit smoke information for the device types supported by
the Model Editor.
Adding smoke information
If you have Advanced Analysis installed, an extra tab, the
Smoke tab, appears next to the Simulation tab. Adding smoke
information involves specifying the maximum operating
conditions for different smoke parameters. Smoke parameters
are the tests that are predefined in the device template file.
These tests are performed between two different nodes of the
device. The node to port mapping information for the device is
available in the Test Node Mapping frame.
The information in the Test Node Mapping frame cannot be
edited for template-based models. For models based on
device characteristic curves, this information is editable. The
Test Node Mapping information is not editable for
template-based models. This is to avoid risk of smoke
information getting out of sync with the smoke test.
See Smoke parameters on page 218
Adding smoke information to PSpice models
Adding smoke information to PSpice models enable you to
use the models for Advanced Analysis smoke run. Using the
Model Editor, you can add smoke information only to the
device types supported by the Model Editor.
212
PSpice User's Guide
Product Version 10.5
Reusing instance models
For template-based models, smoke information is present by
default and is visible in the Smoke Parameters frame. You can
edit this information using the Model Editor. To add smoke
information to a non template-based model, you need to
complete the following steps.
1
From the Models List window, select the model to which
the smoke information is to be added.
Note: If the model that you are trying to edit, has multiple
implementations, you first need to select the
implementation for which changes have to be made, from
the Select Implementation dialog box. This dialog box
lists all the implementations associated with a model. The
changes are saved to the location where original
implementation is stored.
2
From the Model menu choose Add Smoke.
❑
If the model uses the.SUBCKT definition, the Add
Smoke dialog box appears.
a. In the Add Smoke dialog box, specify the device
type.
b. Click OK.
The Test Node Mapping and the Smoke Parameters
frames appear along with the Model Text window that
displays the model definition in the text format.
❑
If the Model uses the .MODEL definition, the Test
Node Mapping and the Smoke Parameters frames
appear along with the Model Text window.
In the Test Node Mapping frame, enter the name of the
port that maps to each Node. The correct node to port
mapping is essential to ensure that smoke analysis gives
correct results. To know more about Test Node Mapping,
see Smoke parameters on page 218.
For the PSpice models with the .MODEL definition, node
names should be the ones that get assigned by part
created using the Model Editor. For the PSpice models
with .SUBCKT definition, node names are defined by the
ports in the subcircuit definition.
PSpice User's Guide
213
Chapter 4
Creating and editing models
Product Version 10.5
3
Enter the maximum operating values for the parameters
in the Smoke Parameters frame.
4
Save the model.
When you save the model, the .LIB and .PRP files are
updated.
Note: When you use the Model Editor to create device
characteristic curves-based PSpice models, the smoke
information is not available by default. After you add the
smoke information, a new file, LIB_NAME.PRP is
created.
Creating template-based PSpice models with smoke information
The steps for creating template-based models with smoke
information are exactly the same as the steps for creating
template-based simulation models. If you have Advanced
Analysis installed, the Smoke tab appears by default. You are
not required to select Add Smoke from the Model menu.
See Example: Creating template-based PSpice model on
page 187
Using the Model Editor to edit smoke information
Open a model with smoke information in the Model Editor. You
can modify the maximum operating values for different smoke
parameters in the Smoke Parameters frame. For models
based on device characteristic curves, you can also change
the port to node mapping in the Test Node Mapping window.
Saving the model will update the .PRP file with the latest
information.
214
PSpice User's Guide
Product Version 10.5
Reusing instance models
Examples: Smoke
Adding smoke information to the D1 diode model
In this example, you will use the Model Editor to add smoke
information to the D1 diode model used in the half-wave
rectifier design explained previously in Example: Creating a
PSpice model based on device characteristic curves on page 180.
To add smoke information, complete the following steps.
1
From the Model menu, choose Add Smoke.
The Test Node Mapping and Smoke Parameters frames
appear.
Note: The Add Smoke command is enabled only if you
have Advanced Analysis installed.
2
In the Test Node Mapping frame, add the following
information.
Node
Port
TERM_AN
1
NODE_AN
1
NODE_CAT 2
You can get the port names by opening the symbol in
Capture.
a. Select the part in Capture.
b. From the Edit menu, choose Part.
c. The symbol view of the part displays. Double-click a
pin.
PSpice User's Guide
215
Chapter 4
Creating and editing models
Product Version 10.5
d. The Name field in the Pin Properties dialog box
displays the port name.
3
In the Smoke Parameters frame, add the following smoke
information.
Property Name
Value
IF
1
VR
30
PDM
1.5
TJ
175
RJC
50
RCA
50
Note: Smoke information is available in the data sheets
provided by the device vendor.
4
To save the changes to the diode model, choose Save
from the File menu.
Once you have modified the D1 diode by adding smoke
information, you can run Smoke analysis on your circuit.
Adding smoke information to the OPA_LOCAL operational amplifier
model
In this example, you will add smoke information to an OPAMP
model created using the Model Editor.
216
PSpice User's Guide
Product Version 10.5
Reusing instance models
See Example: Creating template-based PSpice model on
page 187
You can use the Model Editor to add/edit the smoke
information only if you have Advanced Analysis installed.
The steps in this design example assume that you have
Advanced Analysis installed.
1
Open the Model Editor.
2
Open the LOCAL_LIB library.
3
Select the OPA_LOCAL_3.
Besides the Simulation Parameters and the Model Text
window, a Smoke tab is also displayed.
4
Select the Smoke tab.
The Test Node Mapping and Smoke Parameters frames
are displayed.
5
In the Smoke Parameters frame, specify the maximum
operating conditions for the operational amplifier to match
the values shown in Table 5.
Table 4-6 Modified value of smoke parameters
PSpice User's Guide
Device Max Ops
Value
IPLUS
.05
IMINUS
.05
IOUT
.04
VDIFF
32
VSMAX
32
VSMIN
-.3
VPMAX
.3
VPMIN
.3
VMMAX
-1.5
VMMIN
.3
217
Chapter 4
Creating and editing models
6
Product Version 10.5
Save the model.
The LOCAL_LIB.PRP file will be updated with the smoke
information. The smoke parameters added in this
example are valid for all levels. Even if you delete
OPA_LOCAL_3 from the LOCAL_LIB library, the
LOCAL_LIB.PRP will not be deleted because it contains
smoke information for OPA_LOCAL_1 and
OPA_LOCAL_2.
Smoke parameters
Using the Model Editor, you can add smoke information to the
device types supported by the Model Editor.
When you add smoke information to a device, the following
two frames are displayed in the Model Editor.
■
Test Node Mapping
In this section you specify the port name that must map
to the predefined node names. The predefined terminal
names starting with TERM indicate current nodes, and
those starting with NODE indicate voltage nodes.
■
Smoke Parameters
In this section, you specify the maximum operating
conditions in terms of the values of the smoke
parameters.
The thermal parameters that are common to all device types
supported by the Model Editor are listed below along with their
description.
PDM
Maximum power dissipation
TJ
Maximum junction temperature
RJC
Maximum thermal resistance
(Junction to case thermal resistance)
RCA
218
Maximum thermal resistance (Case to
ambient thermal resistance)
PSpice User's Guide
Product Version 10.5
Smoke parameters
Besides the parameters listed above, there are smoke
parameters specific to a particular class of devices. An
explanation of device-specific smoke parameters and node
names for the Model Editor-supported device types is given
below.
Diode
Test Node Mapping
Node
Port name
TERM_AN
Forward current terminal
NODE_AN
Anode voltage node
NODE_CAT
Cathode voltage node
Smoke Parameters
Smoke
parameter
Maximum operating condition
IF
Maximum Forward Current
(Current through Anode)
VR
Peak Reverse Voltage
(Maximum voltage between
Cathode and Anode)
PSpice User's Guide
219
Chapter 4
Creating and editing models
Product Version 10.5
Bipolar Junction Transistors
Test Node Mapping
Node
Port name
TERM_IC
Collector current terminal
TERM_IB
Base current terminal
NODE_VC
Collector voltage node
NODE_VB
Base voltage node
NODE_VE
Emitter voltage node
Smoke parameters
Smoke
parameter
Maximum operating condition
IB
Maximum base current
IC
Maximum collector current
VCB
Maximum collector-base voltage
(Maximum voltage difference between
Collector and Base)
220
PSpice User's Guide
Product Version 10.5
Smoke parameters
VCE
Maximum collector-emitter voltage
(Maximum voltage difference between
Collector and Emitter)
VEB
Maximum emitter-base voltage
(Maximum voltage difference between
Emitter and Base)
SBSLP
Secondary breakdown slope
Note: Secondary breakdown is the
voltage breakdown between
VC and VE at maximum
collector current.
SBINT
Secondary breakdown intercept
SBTSLP
Secondary breakdown temperature
derating slope
SBMIN
Secondary breakdown derate
percentage at maximum junction
temperature
Magnetic Core
These are a special type of template-based PSpice models
that do not have smoke information. Therefore, the Node
Mapping and Smoke Parameters frames are not available for
these models.
PSpice User's Guide
221
Chapter 4
Creating and editing models
Product Version 10.5
Ins Gate Bipolar Transistor (IGBT)
Test Node Mapping
Node
Port name
TERM_IC
Collector current terminal
TERM_IG
Gate current terminal
NODE_VC
Collector voltage node
NODE_VG
Gate voltage node
NODE_VS
Source voltage node
Smoke parameters
Smoke
parameter
Maximum operating condition
IG
Maximum gate current
IC
Maximum collector current
VCG
Maximum collector-gate voltage
(Voltage between Collector and Gate)
222
PSpice User's Guide
Product Version 10.5
Smoke parameters
VCE
Maximum collector-emitter voltage
(Voltage between Collector and
Emitter)
VGEF
Maximum forward gate-emitter
voltage
(Voltage between Gate and Emitter)
VGER
Maximum reverse gate-emitter
voltage
Junction FET
Test Node Mapping
PSpice User's Guide
Node
Port name
TERM_ID
Depletion current terminal
TERM_IG
Gate current terminal
NODE_VD
Depletion voltage node
NODE_VG
Gate voltage node
NODE_VS
Source voltage node
223
Chapter 4
Creating and editing models
Product Version 10.5
Smoke parameters
Smoke
parameter
Maximum operating condition
ID
Maximum drain current
IG
Maximum forward gate current
VDG
Maximum drain-gate voltage
(Maximum voltage between drain and
gate)
VDS
Maximum drain-source voltage
(Maximum voltage between drain and
source)
VGS
Maximum gate-source voltage
(Maximum voltage between gate and
source)
Operational Amplifier
Test Node Mapping
224
Node
Port name
NODE_POS
Positive voltage source node
(POS)
PSpice User's Guide
Product Version 10.5
Smoke parameters
Node
Port name
NODE_NEG
Negative voltage source node
(NEG)
NODE_VCC
Positive voltage source node
NODE_VEE
Negative voltage source node
NODE_GND
TERM_POS
Positive current terminal
(POS)
TERM_NEG
Negative current terminal
(NEG)
TERM_OUT
Output current terminal (OUT)
Smoke parameters
PSpice User's Guide
Smoke
parameter
Maximum
operating
condition
Stands for...
IPLUS
Maximum input
current (+)
Maximum value of
current at the POS
terminal
IMINUS
Maximum input
current (-)
Maximum value of
current at the NEG
terminal
IOUT
Maximum output
current
Maximum value of
current at the OUT
terminal
VDIFF
Maximum
differential VIN
Absolute voltage
difference between
POS and NEG
VSMAX
Maximum supply
voltage difference
Voltage difference
between NODE_VCC
and NODE_VEE
225
Chapter 4
Creating and editing models
Product Version 10.5
VSMIN
Minimum supply
voltage difference
Voltage difference
between NODE_VEE
and NODE_VCC
VPMAX
Maximum input
voltage (+)
Voltage difference
between NODE_POS
and NODE_VCC
VPMIN
Minimum input
voltage (+)
Voltage difference
between NODE_VEE
and NODE_POS
VMMAX
Maximum input
voltage (-)
Voltage difference
between NODE_NEG
and NODE_VCC
VMMIN
Minimum input
voltage (-)
Voltage difference
between NODE_VEE
and NODE_NEG
MOSFET
Test Node Mapping
226
Node
Port name
TERM_ID
Drain current terminal
TERM_IG
Gate current terminal
PSpice User's Guide
Product Version 10.5
Smoke parameters
Node
Port name
NODE_VD
Drain voltage node
NODE_VG
Gate voltage node
NODE_VS
Source voltage node
Smoke parameters
Smoke
Parameter
Maximum Operating Condition
IG
Maximum forward gate current
ID
Maximum drain current
VDG
Maximum drain-gate voltage
(Maximum difference between
NODE_VD and NODE_VG)
VDS
Maximum drain-source voltage
(Maximum difference between
NODE_VD and NODE_VS)
PSpice User's Guide
VGSF
Maximum forward gate-source
voltage
VGSR
Maximum reverse gate-source
voltage
227
Chapter 4
Creating and editing models
Product Version 10.5
Voltage Regulator
Test Node Mapping
228
Node
Port name
NODE_IN
Input voltage node (IN)
NODE_OUT
Output voltage node (OUT)
NODE_GND
Ground voltage node
(GND)
PSpice User's Guide
Product Version 10.5
Smoke parameters
Darlington Transistor
Test Node Mapping
Node
Port name
TERM_IC
Collector current terminal
TERM_IB
Base current terminal
NODE_VC
Collector voltage node
NODE_VB
Base voltage node
NODE_VE
Emitter voltage node
Smoke parameters
Smoke
parameter
Maximum operating condition
IB
Maximum base current
Max(TERM_IB)
IC
Maximum Collector current
Max(TERM_IC)
VCB
Maximum collector-base voltage
Max(NODE_VC -NODE_VB)
PSpice User's Guide
229
Chapter 4
Creating and editing models
VCE
Product Version 10.5
Maximum collector-emitter voltage
Max(NODE_VC -NODE_VE)
VEB
Maximum emitter-base voltage
Max(NODE_VE -NODE_VB)
SBSLP
Secondary breakdown slope
Note: Secondary breakdown is the
voltage breakdown between
VC and VE at maximum
collector current.
230
SBINT
Secondary breakdown intercept
SBTSLP
Secondary breakdown temperature
derating slope
SBMIN
Secondary breakdown derate
percentage at maximum junction
temperature
PSpice User's Guide
Creating parts for models
5
Chapter overview
This chapter provides information about creating parts for
model definitions, so you can simulate the model from your
design using OrCAD Capture. For general information about
creating parts, refer to the Capture User’s Guide.
Topics are grouped into four areas introduced later in this
overview. If you want to find out quickly which tools to use to
complete a given task and how to start, then:
1
Go to the roadmap in Ways to create parts for models on
page 233.
2
Find the task you want to complete.
3
Go to the sections referenced for that task for more
information about how to proceed.
Background information
These sections provide background on the things you need to
know and do to prepare for creating parts:
PSpice User's Guide
■
What’s different about parts used for simulation? on
page 232
■
Preparing your models for part creation on page 235
231
Chapter 5
Creating parts for models
Product Version 10.5
Task roadmap
This section helps you find the sections in this chapter that are
relevant to the part creation task that you want to complete:
■
Ways to create parts for models on page 233
How to use the tools
These sections explain how to use different tools to create
parts for model definitions:
■
Using the Model Editor to create parts on page 237
■
Basing new parts on a custom set of parts on page 254
Other useful information
These sections explain how to refine part graphics and
properties:
■
Editing part graphics on page 256
■
Defining part properties needed for simulation on
page 262
What’s different about parts used for simulation?
A part used for simulation has these special characteristics:
■
a link to a simulation model
For information on adding simulation models to a model
library, see Chapter 4, “Creating and editing models.”
232
■
a netlist translation
■
modeled pins
■
other simulation properties specific to the part, which can
include hidden pin connections or propagation delay level
(for digital parts)
PSpice User's Guide
Product Version 10.5
Ways to create parts for models
Ways to create parts for models
If you want to...
Then do this...
■
Create parts for a
set of vendor or
user-defined models
saved in a model
library.
■
Change the graphic
standard for an
existing model library.
Automatically create Use the Model Editor1 and
one part each time enable automatic creation
you extract a new
of parts.
model.
■
To find out more, see this...
Use the Model Editor to
Basing new parts on a custom
create parts from a model set of parts on page 254
library.
Using the Model Editor to create
parts on page 237.
For a list of device types that the
Model Editor supports, see
Running the Model Editor alone
on page 165. If the Model Editor
does not support the device type
for the model definition that you
want to create, then you can use
a standard text editor to create a
model definition using the PSpice
.MODEL and .SUBCKT
command syntax. Remember to
configure the new model library
(see Configuring model libraries
on page 202).
Basing new parts on a custom
set of parts on page 254
PSpice User's Guide
233
Chapter 5
Creating parts for models
If you want to...
Then do this...
Create parts for all
the models saved in a
model library.
■
Product Version 10.5
To find out more, see this...
Creating Capture parts for all
models in a library on page 238.
❑
in batch mode
❑
in interactive mode Use the Model Import
Wizard [Capture] to create
parts from a model
library.Use the Model
Import Wizard [Capture] to
create parts from a model
library.
Use the Export to Capture
Part Library command
available in Model Editor to
create parts from a model
library.
1. For a list of device types that the Model Editor supports, see Running the Model Editor alone on
page 165.
234
PSpice User's Guide
Product Version 10.5
Ways to create parts for models
Preparing your models for part creation
If you already have model definitions and want to create parts
for them, you should organize the definitions into libraries
containing similar device types.
To set up a model library for part creation
1
If all of your models are in one file and you wish to keep
them that way, rename the file to:
❑
Reflect the kinds of models contained in the file.
❑
Have the .LIB extension.
Note: Model libraries typically have a .LIB extension.
However, you can use a different file extension as
long as the file format conforms to the standard
model library file format.
2
If each model is in its own file, and you want to
concatenate them into one file, use the DOS copy
command.
Example:
You can append a set of files with .MOD extensions into a
single .LIB file using the DOS command:
copy *.MOD MYLIB.LIB
3
Make sure the model names in your new library do not
conflict with model names in any other model library.
For information on managing model libraries, including
the search order PSpice uses, see Configuring model
libraries on page 202.
PSpice User's Guide
235
Chapter 5
Creating parts for models
Product Version 10.5
Starting the Model Editor
To start the Model Editor alone
1
From the Windows Start menu, point to the Release
OrCAD 10.5 program folder, then choose PSpice
Accessories, Model Editor.
2
From the File menu, choose Open or New, and enter an
existing or new model library name.
3
In the Models List frame, select the name of a model to
display it for editing in the Spec Entry frame.
To start the Model Editor from within Capture
1
In the schematic page editor, select the part whose model
you want to edit.
2
From the Edit menu, choose PSpice Model.
The Model Editor starts with the model loaded for editing.
If you have already started the Model Editor from Capture, and
want to continue working on new models, then:
1
Close the opened model library.
2
Open a new model library.
3
Load a device model or create a new one.
Note: Part creation is disabled, when you launch the Model
Editor from Capture.
236
PSpice User's Guide
Product Version 10.5
Starting the Model Editor
Using the Model Editor to create parts
If you want to create new parts that are not tied to a local
design, open the Model Editor alone. Using Model Editor, you
can create parts in two modes:
❑
Batch mode
❑
Interactive mode
Batch mode of part creation
In this method, you use the Export to Capture Part Library
command from the File menu, to create part symbols for all
models in a simulation library. In this approach, you can view
the symbols only after all the changes have been done and
saved in the .olb file. You need to open the .olb file in
Capture and view the symbols.
To know more about how to use the Export to Capture Part
Library command for part creation see Using batch mode on
page 238.
Interactive mode of part creation
In this mode, you can view the part symbol being attached to
a simulation model before the changes are saved in the
symbol library. You can also update and attach symbols of
your own choice to the models in the library. To create Capture
symbols in an interactive mode, choose Model Import
Wizard [Capture] command, from the File menu.
When you generate part symbols using Model Import wizard,
you can review the symbol shapes before you save the
changes to the part library. This is unlike using Export To
Capture Part Library command, where all the changes are
made to the part library before you can review the symbols by
opening them in Capture.
In the Model Import Wizard, specify the input model library
and the output symbol library and click Next. The model
PSpice User's Guide
237
Chapter 5
Creating parts for models
Product Version 10.5
names and the names of the symbol to be associated with
each model is listed. The symbol shape is visible on the right.
If the users do not make any change and selects the Finish
button, a message box may appear. This message box
appears only if there are models for which symbols could not
be found. To attach a rectangular symbols to such models
click Yes. If you do not wish to attach any symbols select No.
If you select yes, the symbol library generated using the Model
Import Wizard will be exactly same as the .olb generated
using the Export to Capture Part Library command.
To know more about how to create parts using Model Import
Wizard, see Using interactive mode on page 240.
To find out which device types the Model Editor supports, see
Running the Model Editor alone on page 165. If the Model
Editor does not support the device type for the model
definition that you want to create, then you can use a standard
text editor to create a model definition using the PSpice
.MODEL and .SUBCKT command syntax. Remember to
configure the new model library.
Note: The Model Editor is not available with PSpice. A limited
version of the Model Editor is supplied with
PSpice A/D Basics.
Creating Capture parts for all models in a library
Note: Creating parts for all the models in a library is not
supported for libraries that have models with multiple
implementation.
Using batch mode
238
1
Open the Model Editor alone.
From the Windows Start menu, point to the Programs,
Release OrCAD 10.5, and then choose PSpice
Accessories, Model Editor.
2
From the File menu, choose Export to Capture Part
Library.
PSpice User's Guide
Product Version 10.5
Creating Capture parts for all models in a library
The Create Parts for Library dialog box appears.
Tip
Export to Capture Part Library option is available
only if Capture is selected as the schematic editor in
the Options dialog box. To display the Options dialog
box, choose Options from the Tools menu.
3
In the Enter Input Model Library text box, specify the
location of the model library for which the Capture parts
are to be created.
Note: You can use the Browse button to specify a
different location of the .OLB file.
The Enter Output Part Library text box automatically
displays the name and the location of the new .OLB file
to be created. The displayed library name is same as
specified by the user in the Save Part To section of the
OPTIONS dialog box.
4
Click OK to create the part and click OK again to clear the
.ERR log dialog box.
Caution
Recreating an already existing part library, using
the Export to Capture Part Library command does
not overwrite the contents of the part library. Only
the new parts are appended to the library.
Consider a part library, MYLIB.OLB that has two
parts a1 and a2, and a model library, MYLIB.LIB
that has three models a2, b1, and b3. Recreating
MYLIB.OLB from MYLIB.LIB will not delete a1
from MYLIB.OLB. The modified MYLIB.OLB has
four parts, a1, a2, b1, and b2.
PSpice User's Guide
239
Chapter 5
Creating parts for models
Product Version 10.5
Using interactive mode
Important
Model Import Wizard is not recommended if you
want to create new symbol shapes. Using the wizard,
you can only associate existing PSpice model to
existing symbols and vice-versa.You can create new
symbols in OrCAD Capture. To know more about
creating new part symbols or editing existing symbol
graphics, see Editing part graphics on page 256.
Invoke Model Import wizard
From Model Editor
−
From the File drop-down menu, choose Model Import
Wizard [Capture].
Important
To be able to generate Capture parts using Model
Editor, select Capture as the schematic editor in the
Options dialog box.
From Capture
1
Select the Project Manager window in Capture.
2
From the Tools drop-down menu, select Generate Part.
3
In the Generate Part dialog box, select the Pick symbol
manually check box.
4
From the Netlist/source file type drop-down list box, select
PSpice Model Library.
5
To start the symbol generation process, click OK.
1
In the Specify Library page of the Model Import Wizard,
provide inputs.
Using Model Import wizard
240
PSpice User's Guide
Product Version 10.5
Creating Capture parts for all models in a library
a. Specify the name and location of the input model
library (.lib)
b. Specify the name and location of the output part
library (.olb)
Tip
While specifying the library name, you must ensure
that special characters, such as tilde (~), backtick (`),
exclamation mark (!), dollar ($), percentage (%),
caret (^), ampersand (&), plus (+), minus (-), comma
(,), semi colon(;), single quotes ('), and double
quotes (") are not used in the library name.
c. Click the Next button to move to the next step of the
wizard.
When you click the Next button, the Model Import
Wizard automatically starts the process of looking up
symbols for each of the models in the .lib file and
associating the symbols that match the model
definition.
Important
Model Import Wizard uses the model definition
to find a matching symbol for a simulation
model. Therefore, Model Import Wizard can
automatically match symbols only for the device
types supported by the Model Editor. To know
more about these device types, see Model
Editor-supported device types based on device
characteristic curves on page 170.
The matching symbols are stored in the destination part
library specified by you.
2
View the symbols provided by the Model Import Wizard.
The Associate/Replace Symbol page of the wizard lists
the models in the .lib file and the corresponding symbol
names. By default, all models are listed. You can
customize the view to display only those models that have
PSpice User's Guide
241
Chapter 5
Creating parts for models
Product Version 10.5
symbols attached or the models that do not have any
symbols attached.
To display only the models with symbols attached, ensure
that only the Models with symbols check box is
selected.
To display only the models with no symbols attached, only
the Models without symbols check box should be
selected. In this case, the Symbol Name column is blank
.
You can view the attached symbol by selecting a model
from the list of the models with attached symbols. The
symbol shape appears on the right of the wizard.
At this stage, you can complete the process of
associating symbols, and close the Model import wizard
by clicking the Finish button. When you click the Finish
button, you receive a message stating whether you want
to attach rectangular symbols to the models that do not
have symbols attached to them. This message appears
242
PSpice User's Guide
Product Version 10.5
Creating Capture parts for all models in a library
only if the .lib file has some models for which symbols
were not available
In this case, you want rectangular shaped symbols to be
associated with the models, select Yes. To close the
wizard without attaching rectangular symbols to the
models, select No.
Yes
Destination symbol library (.olb) has
symbol looked up by the Model Import
wizard
No
The .olb file has symbols for all the
models in the .lib file.
3
Associate/Replace desired part symbol to a PSpice
model
As the name suggests, the Associate/Replace Symbol
page of the wizard can also be use to review symbol
shapes and if required, attach user-defined symbols to
the models.
The Model import wizard allows you to attach
user-defined symbols to the models without symbols or to
replace the attached symbols with a symbol of your own
choice.
❑
To change the model-symbol association suggested
by Model Import wizard, click the Replace Symbol
button.
❑
To attach a specific symbol to a model for which
matching symbols could not be found, click the
Associate Symbol button.
To attach user-defined symbols to a model:
PSpice User's Guide
243
Chapter 5
Creating parts for models
Product Version 10.5
a. Click the Associate/Replace symbol button.
b. In the Select Matching page of the wizard, specify
the path to the base library
A base library can be defined as the symbol library
(.olb) that contains the desired part symbol. From
the specified library, the Model Import wizard filters
and lists the symbol names that can be attached to
the selected model. You can then select a symbol
from the list, to be associated with the model.
c. Complete the model terminal and symbol pin
mapping.
Use the View Model Test button, to display the model
definition for the selected mode. The pin names of
the selected symbols appear in the Symbol Pin
drop-down list box.
d. Select the Save button to update the destination
symbol file specified in Step 1, with the changes
made by you.
Note: The changes made to the destination library are
irreversible. Once saved, you cannot undo the changes at
the click of a button.
Similarly, you can make associate an existing symbol to any of
the models in the .lib file.
When you use the Model Import wizard to attach a symbol to
a model and vice-versa, following tasks are performed:
244
■
The value of IMPLEMENTATION TYPE property attached
to the symbol is set to PSpice Model.
■
The value of the IMPLEMENTATION property attached to
the symbol is set to the name of the selected model.
(Except in case of leveled models where the level number
is removed.)
■
For models based on device characteristic curves, the
PSPICETEMPLATE property is updated with the
pinname information.
PSpice User's Guide
Product Version 10.5
Setting up automatic part creation
■
For template-based PSpice models, pspice_lnk view is
generated.
Setting up automatic part creation
Automatic part creation from the Model Editor is optional. By
default, automatic part creation is disabled. You can enable it
using the procedure below.
Note: Instead of using the PSpice default part set, you can
use your own set of standard parts. To find out more,
see Basing new parts on a custom set of parts on
page 254.
Tip
In case you want to create a new symbol for only one
model in a library that contains several models, set
up the automatic part creation feature and use the
File, Save command. Every time the file is saved with
automatic part creation enabled, a new symbol is
created for the selected model. All other symbols are
left alone.
To enable automatic part creation for new models
1
In the Model Editor with a library open, choose Options
from the Tools menu.
2
In the Part Creation Setup frame, select Always Create
Part when Saving Model if it is not already checked.
Note: The Always Create Part when Saving Model option
will be disabled if you start the Model Editor from Capture.
3
Select the Pick symbols Manually check box, to ensure
that Model Import Wizard is invoked every time you
generate a part symbol for a model.
Note: In this case, the Specify Library page of the wizard
is not required and is therefore, not visible. The
Associate/Replace symbol page will be invoked.
PSpice User's Guide
245
Chapter 5
Creating parts for models
4
Product Version 10.5
In the Save Part To frame, define the name of the part
library for the new part. Choose one of the following:
❑
Part library path same as model library to create or
open the *.OLB file that has the same filename as
the open model library (*.LIB).
For example, if the model library is named
MYPARTS.LIB, then the Model Editor creates the
part library named MYPARTS.OLB.
❑
User-defined part library, and then enter a library
name in the part Library Name text box.
Example
The examples covered in this section demonstrate the steps
involved in creating a part using the Model Editor. The
examples covered in this section are:
■
Creating parts in the batch mode
■
Creating parts using interactive mode
Creating parts in the batch mode
This example is the continuation of the Example: Creating
template-based PSpice model used in Chapter 4, “Creating
and editing models.”
The tasks covered in this example are:
246
■
Creating parts for the models in a model library using the
Export to Capture Part Library command.
■
Using the Model Editor created part in a schematic
design.
❑
Passing parameters to a simulation model from the
schematic.
❑
Using model with multiple levels of simulation
parameters. Difference in the use model for Model
Editor-created model and OrCAD supplied model
PSpice User's Guide
Product Version 10.5
Example
In this example, you will create parts for the simulation models
in the LOCAL_LIB model library. The LOCAL_LIB library
created as part of Example: Creating template-based PSpice
model has a template-based model of an operational
amplifier, OPA_LOCAL.
Creating Capture parts
To create Capture parts for all the models in the
LOCAL_LIB.LIB library:
1
From the File menu choose Export to Capture Part library.
Note: The Export to Capture Part Library option is
available only if you select Capture as the schematic
editor in the Options dialog box.
2
In the Create Parts for Library dialog box, ensure that the
input model library is LOCAL_LIB.LIB and save the new
Capture part library (LOCAL_LIB.OLB) in the same
location as the model library.
3
Click OK, to create parts.
The LOCAL_LIB.OLB that gets created has one part,
OPA_LOCAL, with the LEVEL property is attached to the part
symbol. By default, the value of the LEVEL property is set to 1.
Template-based operational amplifier model created using the
Model Editor has multiple level support. If the value of the
LEVEL property is set to 1, first level of simulation parameters
are used while simulating the model. Similarly, if the LEVEL
value set to 2, second level of simulation parameters are used,
and so on.
Using the Model Editor created parts in a design
In this section you will create an amplifier using two internally
compensated operational amplifiers. One of the Operational
Amplifier, CA1458, is supplied along with PSpice in the
OPA.LIB model library, and the second Operational Amplifier
used is OPA_LOCAL, created using the Model Editor. Both the
models are template-based and both support multiple levels of
simulation parameters.
PSpice User's Guide
247
Chapter 5
Creating parts for models
Product Version 10.5
1
In Capture, create a new project FUNC_GEN.OPJ, and
include LOCAL_LIB.LIB as one of the model library.
2
Create a circuit as shown in the figure below.
The model CA1458, is a multi-level model and by default,
the model level is 3. The LEVEL property for the
OPA_LOCAL model is set to 2.
Note: You can also pick the design from,
...\tools\pspice\tutorial\capture\modeleditor.
3
To simulate the circuit, choose Run from the PSpice
menu in Capture.
Changing the level of simulation parameters used in the design
We will now modify the circuit design, such that level 2
simulation parameters are used for CA1458 and level 3
simulation parameters are used for the OPA_LOCAL model,
created using the Model Editor.
248
PSpice User's Guide
Product Version 10.5
Example
Changing the level for CA1458
To change the level of simulation parameters for CA1458 from
3 to 2,
1
Select the part CA1458.
2
From the Edit menu, choose Properties.
3
In the Property editor dialog box, change the value of
LEVEL property from 3 to2.
4
Click Apply and close the Property Editor.
Similarly, change the value of the LEVEL property on
OPA_LOCAL from 2 to 3.
You can now simulate the circuit using PSpice or PSpice
Advanced Analysis.
Changing Simulation Properties from Capture
For all the editable simulation properties, you can specify the
value of simulation parameters from Capture.
1
Select OPA_LOCAL.
2
From the Edit menu, choose Properties.
3
In the Property Editor dialog box, select New Row.
4
In the Add New Row dialog box, enter the name of the
simulation parameter in the Name text box. Enter VOS.
5
In the Value text box, add the value of the simulation
parameter as 2e-3 and select OK.
6
To make the property and its value visible, first select
property row and then select the Display button in the
Property Editor dialog box.
7
Specify the Display Format. Select Name and Value.
8
Select Apply and close the dialog box.
The simulation parameter and its value appear in the Capture.
If you now simulate the design, the simulation parameter value
specified in Capture will be used.
PSpice User's Guide
249
Chapter 5
Creating parts for models
Product Version 10.5
Creating parts using interactive mode
In this section, we will use the Model Import wizard to create
models stored in a user defined library, MYLIB. This library
consists of four simulation models. These are LM339; which is
a voltage comparator macro model subcircuit, INA105E;
which is an operational amplifier plus precision resistor
network, LF442A/NS; which is a JFET OPAMP, and mybjt;
which is a Bipolar Junction Transistor.
Launch Model Import Wizard
1
From the File drop-down menu in Model Editor, choose
Model Import Wizard [Capture].
Provide Inputs
1
In the Specify Library page of the wizard, specify the
location of MYLIB.LIB.
2. Specify the name of the part library in which the part
symbols generated by the Wizard are to be stored.
250
PSpice User's Guide
Product Version 10.5
Example
You can either specify the name of an existing .olb file
or create a new .olb file.
When you specify the name of an existing .olb file, you
also need to specify if symbols should be created for all
the models in the model library while replacing the
existing symbols, or whether part symbols are to be
created only for the models without the symbols.
The name and the location of the destination symbol
library gets populated by default. For the current example,
accept the default name, mylib.olb and click Next.
Depending on the model definition, the Model Import
wizard could locate appropriate part symbol for the BJT
model only. The named of the symbol attached to the
mybjt model, is listed in the Symbol Name column and
the symbol shape is also visible.
3
You can now complete one of the following steps:
a. Close the wizard without attaching any symbols of
the rest of the three models in mylib.lib.
PSpice User's Guide
251
Chapter 5
Creating parts for models
Product Version 10.5
b. Close the wizard, after Model Import wizard attaches
rectangular symbols to rest of the models in
mylib.lib.
c. Use the Model Import wizard to select and attach an
existing symbol shape to one or all the models in
mylib.lib.
To execute the first two options, click the Finish button. In
the message box that appears, select No to close the
library and Yes to attach rectangular symbols and then
close the library.
Associating desired part symbol to a PSpice model
We will now use the Model Import wizard to attach an existing
user-defined, symbol to LF442A/NS; which is a JFET OPAMP.
LF442A is a Dual Low Power JFET Input Operational
Amplifier, downloaded from National Semiconductor's web
site. We will pick up the symbol from the symbol library
opamp.olb, which contains symbols for different types of
OPAMPs.
1
In the Associate/Replace page of the Model Import
Wizard, select LF442A/NS, and click Associate Symbol.
2
In the Select Matching page of the wizard, specify the
name and the location of opamp.olb.
All symbols that match the model definition are listed in
the Matching Symbols list.
252
3
From the Matching symbols list, select LM158 and click
Next.
4
Before you start mapping the model terminals to the
symbol pin names, click the View Model Text button.
PSpice User's Guide
Product Version 10.5
Example
The model definition of LF442A/NS appears in a different
window.
5
6
Map the model terminals and the symbol pin names.
Model terminal
Mapped to Symbol Pin
1
+
2
-
99
V+
50
V-
28
OUT
To attach the symbol to LF442A/NS, click the Save
Symbol button.
The name of the symbol attached to the model appears
in the Symbol Name list.
You have successfully attached a symbol to the selected
model. Similarly, you can attach models for the other two
symbols as well.
Note: You can use the Model Import wizard to replace a
symbol attached to a model with another symbol. To do
this, select the model that has a symbol attached to it,
and click the Replace Symbol button.
PSpice User's Guide
253
Chapter 5
Creating parts for models
Product Version 10.5
Important
Model Import Wizard can be invoked from Capture to
associate a PSpice model to an existing Capture
Symbol. To know more about associating PSpice
model to a Capture symbol, see OrCAD Capture
User Guide.
Basing new parts on a custom set of parts
If you are using the Model Editor to automatically generate
parts for model definitions, and you want to base the new
parts on a custom graphic standard (rather than the PSpice
default parts), then you can change which underlying parts
either application uses by setting up your own set of parts.
Note: If you use a custom part set, the Model Editor always
checks the custom part library first for a part that
matches the model definition. If none can be found,
they use the PSpice default part instead.
To create a custom set of parts for automatic part
generation
1
Create a part library with the custom parts.
Be sure to name these parts by their device type as
shown in Table 5-1 and Table 5-2; this is how the Model
Editor determines which part to use for a model definition.
For more information on creating parts, refer to the
OrCAD Capture User’s Guide.
Table 5-1 Symbol Names for custom symbol generation for regular PSpice models
For this device type...
Use this symbol For this device type...
name...
Use this symbol
name...
Bipolar transistor: LPNP
LPNP
Magnetic core
CORE
Bipolar transistor: NPN
NPN
MOSFET: N-channel
NMOS
Bipolar transistor: PNP
PNP
MOSFET: P-channel
PMOS
254
PSpice User's Guide
Product Version 10.5
Basing new parts on a custom set of parts
Table 5-1 Symbol Names for custom symbol generation for regular PSpice models
For this device type...
Use this symbol For this device type...
name...
Use this symbol
name...
Capacitor1
CAP
OPAMP: 5-pin
OPAMP5
Darlington: N-channel
DARNPN
OPAMP: 7-pin
OPAMP7
Darlington: P-channel
DARPNP
Resistor1
RES
Diode
DIODE
Switch:
voltage-controlled1
VSWITCH
GaAsFET1
GASFET
Transmission line1
TRN
IGBT: N-channel
NIGBT
Voltage comparator
VCOMP
Inductor1
IND
Voltage comparator: 6 pin VCOMP6
JFET: N-channel
NJF
Voltage reference
VREF
JFET: P-channel
PJF
Voltage regulator
VREG
1. Does not apply to the Model Editor.
Table 5-2 Symbol Names for Custom Symbol Generation for template-based Models
For this device type...
Use this symbol For this device type...
name...
Bipolar transistor: LPNP
Use this symbol
name...
Magnetic core
AACORE
Bipolar transistor: NPN
AANPN3
MOSFET: N-channel
AANMOSFET3
Bipolar transistor: PNP
AAPNP3
MOSFET: P-channel
AAPMOSFET3
Capacitor1
CAP
OPAMP: 5-pin
AA5_PIN_OPAMP
Darlington: N-channel
AADARNPN3
OPAMP: 7-pin
AA7_PIN_OPAMP
Darlington: P-channel
AADARPNP3
Resistor1
Diode
AADIODE
Switch:
voltage-controlled1
GaAsFET1
IGBT: N-channel
Inductor1
PSpice User's Guide
Transmission line1
AANIGBT3
Voltage comparator
Voltage comparator: 6
pin
255
Chapter 5
Creating parts for models
Product Version 10.5
Table 5-2 Symbol Names for Custom Symbol Generation for template-based Models
For this device type...
Use this symbol For this device type...
name...
JFET: N-channel
AANCHANNEL3
Voltage reference
JFET: P-channel
AANPHANNEL3
Voltage regulator
Use this symbol
name...
AAVREG
1. Does not apply to the Model Editor.
2
For each custom part, set its IMPLEMENTATION
property to `M where ` is a back-single quote or grave
character.
This tells the Model Editor to substitute the correct model
name.
To base new parts on custom parts using the Model
Editor
1
In the Model Editor with the library open, choose Part
Creation Setup from the Options menu, and enable
automatic part creation as described in To enable
automatic part creation for new models on page 245.
2
In the Base Parts On frame, enter the name of the
existing part library (*.OLB) that contains your custom
parts.
3
Click OK.
Editing part graphics
If you created parts using the Model Editor, and you want to
make further changes, the following sections explain a few
important things to remember when you edit the parts.
How Capture places parts
When placing parts on the schematic page, the schematic
page editor uses the grid as a point of reference for different
256
PSpice User's Guide
Product Version 10.5
Editing part graphics
editing activities. The part’s pin ends are positioned on the grid
points.
grid point
part body border
To edit a part in a library
1
From Capture’s File menu, point to Open, then choose
Library.
2
Select the library that has the part you want to edit.
The library opens and displays all its parts.
3
Double-click the part you want to edit.
The part appears in the part editor.
4
Edit the part.
You can resize it, add or delete graphics, and add or
delete pins. For more information about specific part
editing tasks, refer to the OrCAD Capture User’s
Guide.
5
After you have finished editing the part, from the File
menu, choose Save to save the part to its library.
Here are the things to check when editing part properties:
PSpice User's Guide
■
Does the PSPICETEMPLATE specify the correct number
of pins/nodes?
■
Are the pins/nodes in the PSPICETEMPLATE specified
in the proper order?
257
Chapter 5
Creating parts for models
■
Product Version 10.5
Do the pin/node names in the PSPICETEMPLATE match
the pin names on the part?
Defining grid spacing
Grid spacing for graphics
The grid, denoted by evenly spaced grid points, regulates the
sizing and positioning of graphic objects and the positioning of
pins. The default grid spacing with snap-to-grid enabled is
0.10", and the grid spacing is 0.01".
You can turn off the grid spacing when you need to draw
graphics in a tighter space.
To edit the part graphics
1
In Capture’s part editor, display the part you want to edit.
2
Select the line, arc, circle, or other graphic object you
want to change, and do any of the following:
❑
To stretch or shrink the graphic object, click and drag
one of the size handles.
❑
To move the entire part graphic, click and drag the
edge of the part.
The part body border automatically changes to fit the
size of the part graphic.
3
After you have finished editing the part, from the File
menu, choose Save to save the part to its library.
Note: When changing part graphics, check to see that all pins
are on the grid.
Grid spacing for pins
The part editor always places pins on the grid, even when the
snap-to-grid option is turned off. The size of the part is relative
to the pin-to-pin spacing for that part. That means that pins
258
PSpice User's Guide
Product Version 10.5
Attaching models to parts
placed one grid space apart in the part editor are displayed as
one grid space apart in the schematic page editor.
Pins must be placed on the grid at integer multiples of the grid
spacing. Because the default grid spacing for the Schematic
Page Grid is set at 0.10", you will achieve the best results by
setting pin spacing in the Part and Symbol Grid at 0.10"
intervals from the origin of the part and at least 0.10" from any
adjacent pins. For more information about grid spacing and
pin placement, refer to the OrCAD Capture User’s Guide.
The part editor considers pins that are not placed at integer
multiples of the grid spacing from the origin as off-grid, and a
warning appears when you try to save the part.
Here are two guidelines:
■
Make sure Pointer Snap to Grid is enabled when editing
part pins and editing schematic pages so you can easily
make connections.
■
Make sure the Part and Symbol Grid spacing matches
the Schematic Page Grid spacing.
Note: Pin changes that alter the part template can occur if
you either:
❑
change pin names
or
❑
delete pins
In these cases you must adjust the value of the part’s
PSPICETEMPLATE property to reflect these changes. To
find out how, see Pin callout in subcircuit templates on
page 270.
Attaching models to parts
If you create parts and want to simulate them, you need to
attach model implementations to them. If you created your
parts using any of the methods discussed in this chapter, then
your part will have a model implementation already attached
to it.
PSpice User's Guide
259
Chapter 5
Creating parts for models
Product Version 10.5
MODEL
The IMPLEMENTATION property defines the name of the
model that PSpice must use for simulation. When attaching
this implementation, this rule applies:
■
The Implementation name should match the name of the
.MODEL or .SUBCKT definition of the simulation model
as it appears in the model library (*.LIB).
Example:
If your design includes a 2N2222 bipolar transistor with a
.MODEL name of Q2N2222, then the Implementation name
for that part should be Q2N2222.
Note: Make sure that the model library containing the
definition for the attached model is configured in the list
of libraries for your project. See Configuring model
libraries on page 202 for more information.
For more information on model editing in general, see
Chapter 4, “Creating and editing models.” For specific
information on changing model references, see Changing the
model reference to an existing model definition on page 199.
To attach a model implementation
1
In the schematic page editor, double-click a part to
display the Parts spreadsheet of the Property Editor.
Assume the spreadsheet is displayed in columns and
follow the instructions below.
2
Click on the empty cell under the Implementation Type
column.
A drop-down list appears in the cell.
3
From the Implementation Type drop-down list, select
PSpice Model.
4
Click on the empty cell under the Implementation column,
and type the name of the model to attach to the part.
Note: You do not need to enter an Implementation Path
260
PSpice User's Guide
Product Version 10.5
Attaching models to parts
because PSpice searches for the model in the list of
model libraries you configure for this project.
5
Click Apply to update the design, then close the Parts
spreadsheet.
Caution
In case you want to reuse the part symbol that
was originally attached to a characteristic
curve-based model, with a template-based
simulation model, you must delete the
PSPICETEMPLATE property from the part
symbol.
Example:
Consider a scenario where you have two simulation
models for a bipolar transistor, with the same name
2n2222 in two different libraries. First simulation model is
based on characteristic curves and the second based on
PSpice templates. Both the simulation models have same
name, therefore the same value for the
IMPLEMENTATION property.
The simulation model based on characteristic curves,
which is of .MODEL type, is used in a schematic design.
The part symbol for the bipolar transistor will have the
IMPLEMENTAION property set to Q2n2222 and the
PSPICETEMPLATE property attached to it. Now modify
the BJT symbol by attaching a template-based model to
the symbol. The value of the IMPLEMENTATION property
will not change because the name of the template-based
model is same as that of the characteristic curves-based
model. Therefore, to ensure that the correct model is
used during simulation, you must delete the
PSPICETEMPLATE property from the part symbol and
configure the library containing the template-based BJT
model.
Note: You can check whether the right model is being
used or not, by viewing the simulation netlist generated by
PSPice. The simulation netlist for a .MODEL type BJT
model starts with Q, where as the simulation netlist for a
.SUBCKT model starts with X.
PSpice User's Guide
261
Chapter 5
Creating parts for models
Product Version 10.5
Defining part properties needed for simulation
If you created your parts using any of the methods discussed
in this chapter, then your part will have these properties
already defined for it:
■
PSpice PSPICETEMPLATE for simulation
■
PART and REFDES for identification
You can also add other simulation-specific properties for
digital parts: IO_LEVEL, MNTYMXDLY, and
PSPICEDEFAULTNET (for pins).
Example:
If you create a part that has electrical behavior described by
the subcircuit definition that starts with:
.SUBCKT 7400 A B Y
+ optional: DPWR=$G_DPWR DGND=$G_DGND
+ params: MNTYMXDLY=0 IO_LEVEL=0
then the appropriate part properties are:
IMPLEMENTATION = 7400
MNTYMXDLY = 0
IO_LEVEL = 0
PSPICETEMPLATE = X^@REFDES %A %B %Y %PWR %GND
@MODEL PARAMS:IO_LEVEL=@IO_LEVEL
MNTYMXDLY=@MNTYMXDLY
Note: For clarity, the PSPICETEMPLATE property value is
shown here in multiple lines; in a part definition, it is
specified in one line (no line breaks).
To edit a property needed for simulation:
262
1
In the schematic page editor, select the part to edit.
2
From the Edit menu, choose Properties to display the
Parts spreadsheet of the Property Editor.
3
Click in the cell of the column you want to change (for
example, PSPICETEMPLATE), or click the New button to
add a property (and type the property name in the Name
text box).
4
If needed, type a value in the Value text box.
PSpice User's Guide
Product Version 10.5
Defining part properties needed for simulation
5
Click Apply to update the design, then close the
spreadsheet.
Table 5-3
To find out more about
this property...
See this...
PSPICETEMPLATE
PSPICETEMPLATE on
page 263
IO_LEVEL
IO_LEVEL on page 272
MNTYMXDLY
MNTYMXDLY on page 273
PSPICEDEFAULTNET
PSPICEDEFAULTNET on
page 274
PSPICETEMPLATE
The PSPICETEMPLATE property defines the PSpice syntax
for the part’s netlist entry. When creating a netlist, Capture
substitutes actual values from the circuit into the appropriate
places in the PSPICETEMPLATE syntax, then saves the
translated statement to the netlist file.
Caution
The PSPICETEMPLATE property is required only
for models based on device characteristic curves.
For template-based models, netlisting is done
using the PORT_ORDER information available in
the device property file.
Note: The PSPICETEMPLATE property is not required
with template-based models. Therefore, while modifying
a design, if you attach a template-based model to a part
originally attached to a characteristic curve based model,
then besides changing the Implementation property, you
must also delete the PSPICETEMPLATE property.
Any part that you want to simulate must have a defined
PSPICETEMPLATE property. These rules apply:
PSpice User's Guide
263
Chapter 5
Creating parts for models
Product Version 10.5
■
The pin names specified in the PSPICETEMPLATE
property must match the pin names on the part.
■
The number and order of the pins listed in the
PSPICETEMPLATE property must match those for the
associated .MODEL or .SUBCKT definition referenced for
simulation.
■
The first character in a PSPICETEMPLATE must be a
PSpice device letter appropriate for the part (such as Q
for a bipolar transistor).
See Passive parts on page 117 and Breakout parts on
page 118 for a list of device types and PSpice device
letters.
Device types and PSpice device letters are also listed in
the online PSpice A/D Reference Guide.
Caution
Creating parts not intended for simulation
Some part libraries contain parts designed only
for board layout; PSpice cannot simulate these
parts. This means they do not have
PSPICETEMPLATE properties or that the
PSPICETEMPLATE property value is blank.
PSPICETEMPLATE syntax
The PSPICETEMPLATE contains:
■
regular characters that the schematic page editor
interprets verbatim
■
property names and control characters that the
schematic page editor translates
Regular characters in templates
Regular characters include the following:
■
264
alphanumerics
PSpice User's Guide
Product Version 10.5
Defining part properties needed for simulation
■
any keyboard part except the special syntactical parts
used with properties (@ & ? ~ #).
■
white space
An identifier is a collection of regular characters of the form:
alphabetic character [any other regular character]*.
Property names in templates
Property names are preceded by a special character as
follows:
[ @ | ? | ~ | # | & ]<identifier>
The schematic page editor processes the property according
to the special character as shown in the following table.
Table 5-4
This syntax...1
Is replaced with this...
@<id>
Value of <id>. Error if no <id> attribute or
if no value assigned.
&<id>
Value of <id> if <id> is defined.
?<id>s...s
Text between s...s separators if <id> is
defined.
?<id>s...ss...s Text between the first s...s separators if
<id> is defined, else the second s...s
clause.
~<id>s...s
Text between s...s separators if <id> is
undefined.
~<id> s...ss...s Text between the first s...s separators if
<id> is undefined, else the second s...s
clause.
#<id>s...s
Text between s...s separators if <id> is
defined, but delete rest of template if <id>
is undefined.
1. s is a separator character
PSpice User's Guide
265
Chapter 5
Creating parts for models
Product Version 10.5
Separator characters include commas (,), periods (.),
semicolons (;), forward slashes (/), and vertical
bars ( | ). You must always use the same character to specify
an opening-closing pair of separators.
Example: The template fragment ?G|G=@G||G=1000| uses
the vertical bar as the separator between the if-then-else parts
of this conditional clause. If G has a value, then this fragment
translates to G=<G property value>. Otherwise, this
fragment translates to G=1000.
Note: You can use different separator characters to nest
conditional property clauses.
The ^ character in templates
The schematic page editor replaces the ^ character with the
complete hierarchical path to the device being netlisted.
The \n character sequence in templates
The part editor replaces the character sequence \n with a new
line. Using \n, you can specify a multi-line netlist entry from a
one-line template.
The % character and pin names in templates
Pin names are denoted as follows:
%<pin name>
where pin name is one or more regular characters.
The schematic page editor replaces the %<pin name> clause
in the template with the name of the net connected to that pin.
The end of the pin name is marked with a separator (see
Property names in templates on page 265). To avoid name
266
PSpice User's Guide
Product Version 10.5
Defining part properties needed for simulation
conflicts in PSpice, the schematic page editor translates the
following characters contained in pin names.
Table 5-5
This pin name
character...
Is replaced with this...
<
l (L)
>
g
=
e
\XXX\
XXXbar
Note: To include a literal % character in the netlist, type %% in
the template.
Caution
Recommended scheme for netlist templates
Templates for devices in the part library start with
a PSpice device letter, followed by the
hierarchical path, and then the reference
designator (REFDES) property. We recommend
that you adopt this scheme when defining your
own netlist templates.
Example: R^@REFDES ... for a resistor
PSPICETEMPLATE examples
Simple resistor (R) template
The R part has:
■
two pins: 1 and 2
■
two required properties: REFDES and VALUE
Template
R^@REFDES %1 %2 @VALUE
PSpice User's Guide
267
Chapter 5
Creating parts for models
Product Version 10.5
Sample translation
R_R23 abc def 1k
where REFDES equals R23, VALUE equals 1k, and R is
connected to nets abc and def.
Voltage source with optional AC and DC specifications
(VAC) template
The VAC part has:
■
two properties: AC and DC
■
two pins: + and -
Template
V^@REFDES %+ %- ?DC|DC=@DC| ?AC|AC=@AC|
Sample translation
V_V6 vp vm DC=5v
where REFDES equals V6, VSRC is connected to nodes
vp and vm, DC is set to 5v, and AC is undefined.
Sample translation
V_V6 vp vm DC=5v AC=1v
where, in addition to the settings for the previous
translation, AC is set to 1v.
Parameterized subcircuit call (X) template
Suppose you have a subcircuit Z that has:
■
two pins: a and b
■
a subcircuit parameter: G, where G defaults to 1000 when
no value is supplied
To allow the parameter to be changed on the schematic page,
treat G as an property in the template.
Template
X^@REFDES %a %b Z PARAMS: ?G|G=@G|
~G|G=1000|
268
PSpice User's Guide
Product Version 10.5
Defining part properties needed for simulation
Note: For clarity, the PSPICETEMPLATE property value is
shown here in multiple lines; in a part definition, it is
specified in one line (no line breaks).
Equivalent template (using the if...else form)
X^@REFDES %a %b Z PARAMS: ?G|G=@G||G=1000|
Sample translation
X_U33 101 102 Z PARAMS: G=1024
where REFDES equals U33, G is set to 1024, and the
subcircuit connects to nets 101 and 102.
Sample translation
X_U33 101 102 Z PARAMS: G=1000
where the settings of the previous translation apply
except that G is undefined.
Digital stimulus parts with variable width pins template
For a digital stimulus device template (such as that for a
DIGSTIM part), a pin name can be preceded by a * character.
This signifies that the pin can be connected to a bus and the
width of the pin is set to be equal to the width of the bus.
Template
U^@REFDES STIM(%#PIN, 0) %*PIN
\n+ STIMULUS=@STIMULUS
where #PIN refers to a variable width pin.
Note: For clarity, the PSPICETEMPLATE property value is
shown here in multiple lines; in a part definition, it is
specified in one line (no line breaks).
Sample translation
U_U1 STIM(4,0) 5PIN1 %PIN2 %PIN3 %PIN4
+ STIMULUS=mystim
where the stimulus is connected to a four-input bus,
a[0-3].
PSpice User's Guide
269
Chapter 5
Creating parts for models
Product Version 10.5
Pin callout in subcircuit templates
The number and sequence of pins named in a template for a
subcircuit must agree with the definition of the subcircuit
itself—that is, the node names listed in the .SUBCKT
statement, which heads the definition of a subcircuit. These
are the pinouts of the subcircuit. To find out how to define
subcircuits, refer to the .SUBCKT command in the online
PSpice Reference Guide.
Example:
Consider the following first line of a (hypothetical) subcircuit
definition:
.SUBCKT SAMPLE 10 3 27 2
The four numbers following the name SAMPLE—10, 3, 27,
and 2—are the node names for this subcircuit’s pinouts.
Now suppose that the part definition shows four pins:
IN+
OUT+
IN-
OUT-
The number of pins on the part equals the number of nodes in
the subcircuit definition.
If the correspondence between pin names and nodes is as
follows:
Table 5-6
This node
name...
Corresponds to this pin name...
10
IN+
3
IN-
27
OUT+
2
OUT-
then the template looks like this:
X^@REFDES %IN+ %IN- %OUT+ %OUT- @MODEL
270
PSpice User's Guide
Product Version 10.5
Defining part properties needed for simulation
The rules of agreement are outlined in Figure 5-1.
Number of nodes in first line
of subcircuit definition
must
equal
Sequence of nodes in first line
of subcircuit definition
must
match
Number of pins called out
in template
must
equal
Number of modeled* pins
shown in part
Sequence of pins called out
in template
Names of pins called out
in template
must
match
Names of modeled* pins
shown in part
* Unmodeled pins may appear on a part (like the two voltage offset pins on a 741 opamp part).
These pins are not netlisted and do not appear on the template.
Figure 5-1 Rules for pin callout in subcircuit templates
PSpice User's Guide
271
Chapter 5
Creating parts for models
Product Version 10.5
IO_LEVEL
All digital parts provided in the PSpice libraries have an
IO_LEVEL property.
The IO_LEVEL property defines what level of interface
subcircuit model PSpice must use for a digital part that is
connected to an analog part. To find out more about interface
subcircuits, see Interface subcircuit selection by PSpice on
page 579.
To use the IO_LEVEL property with a digital part
1
Add the IO_LEVEL property to the part and assign a
value shown in the table below.
Table 5-7
Assign this
value...
To use this interface
subcircuit (level)...
0
circuit-wide default
1
AtoD1 and DtoA1
2
AtoD2 and DtoA2
3
AtoD3 and DtoA3
4
AtoD4 and DtoA4
2
Use this property in the PSPICETEMPLATE property
definition (IO_LEVEL is also a subcircuit parameter used
in calls for digital subcircuits).
Example:
PSPICETEMPLATE=X^@REFDES %A %B %C %D %PWR %GND
@MODEL PARAMS:\n+
IO_LEVEL=@IO_LEVEL
MNTYMXDLY=@MNTYMXDLY
Note: For clarity, the PSPICETEMPLATE property value is
shown here in multiple lines; in a part definition, it is
specified in one line (no line breaks).
272
PSpice User's Guide
Product Version 10.5
Defining part properties needed for simulation
MNTYMXDLY
All digital parts provided in the PSpice libraries have a
MNTYMXDLY property.
The MNTYMXDLY property defines the digital propagation
delay level that PSpice must use for a digital part. To find out
more about propagation delays, see Timing characteristics on
page 339 and Selecting propagation delays on page 560.
To use the MNTYMXDLY property with a digital part
1
Add the MNTYMXDLY property to the part and assign a
value shown in the table below.
Table 5-8
2
Assign this
value...
To use this propagation delay...
0
circuit-wide default
1
minimum
2
typical
3
maximum
4
worst-case (min/max)
Use this property in the PSPICETEMPLATE property
definition (MNTYMXDLY is also a subcircuit parameter
used in calls for digital subcircuits).
Example:
PSPICETEMPLATE=X^@REFDES %A %B %C %D %PWR %GND
@MODEL PARAMS:\n+
IO_LEVEL=@IO_LEVEL
MNTYMXDLY=@MNTYMXDLY
Note: For clarity, the PSPICETEMPLATE property value is
shown here in multiple lines; in a part definition, it is
specified in one line (no line breaks).
PSpice User's Guide
273
Chapter 5
Creating parts for models
Product Version 10.5
PSPICEDEFAULTNET
The PSPICEDEFAULTNET pin property defines the net name
to which a hidden (invisible) pin is connected. Hidden pins are
typically used for power and ground on digital parts.
To use the PSPICEDEFAULTNET property with a digital
part
1
For each PSPICEDEFAULTNET property, assign the
name of the digital net to which the pin is connected.
Example:
If power (PWR) and ground (GND) pins of a digital part
connect to the digital nets $G_DPWR and $G_DGND,
respectively, then the PSPICEDEFAULTNET properties
for these pins are:
PSPICEDEFAULTNET=$G_DPWR
PSPICEDEFAULTNET=$G_DGND
2
Use the appropriate hidden pin name in the
PSPICETEMPLATE property definition.
Example:
If the name of the hidden power pin is PWR and the name
of the hidden ground pin is GND, then the template might
look like this:
PSPICETEMPLATE=X^@REFDES %A %B %C %D %PWR %GND
@MODEL PARAMS:\n+
IO_LEVEL=@IO_LEVEL
MNTYMXDLY=@MNTYMXDLY
Note: For clarity, the PSPICETEMPLATE property value is
shown here in multiple lines; in a part definition, it is
specified in one line (no line breaks).
274
PSpice User's Guide
Analog behavioral modeling
6
Chapter overview
This chapter describes how to use the Analog Behavioral
Modeling (ABM) feature of PSpice. This chapter includes the
following sections:
PSpice User's Guide
■
Overview of analog behavioral modeling on page 276
■
The ABM.OLB part library file on page 277
■
Placing and specifying ABM parts on page 278
■
ABM part templates on page 280
■
Control system parts on page 281
■
PSpice-equivalent parts on page 307
■
Cautions and recommendations for simulation and
analysis on page 320
■
Basic controlled sources on page 326
275
Chapter 6
Analog behavioral modeling
Product Version 10.5
Overview of analog behavioral modeling
You can use the Analog Behavioral Modeling (ABM) feature of
PSpice to make flexible descriptions of electronic components
in terms of a transfer function or lookup table. In other words,
a mathematical relationship is used to model a circuit
segment, so you do not need to design the segment
component by component.
The part library contains several ABM parts that are classified
as either control system parts or as PSpice-equivalent parts.
See Basic controlled sources on page 326 for an introduction
to these parts, how to use them, and the difference between
parts with general-purpose application and parts with
special-purpose application.
Control system parts are defined with the reference voltage
preset to ground so that each controlling input and output are
represented by a single pin in the part. These are described in
Control system parts on page 281.
PSpice-equivalent parts reflect the structure of the PSpice E
and G device types, which respond to a differential input and
have double-ended output. These are described in
PSpice-equivalent parts on page 307.
You can also use the Device Equations Developer’s Kit for
modeling of this type, but we recommend using the ABM
feature wherever possible. With the Device Equations
Developer’s Kit, the PSpice source code is actually modified.
While this is more flexible and produces faster results, it is also
much more difficult to use and to troubleshoot. Also, any
changes you make using the Device Equations Developer’s
Kit must be made to all new PSpice updates you install.
Note: The Device Equations Developer’s Kit is available to
qualified customers only. Please contact PSpice
Customer Support for qualification criteria.
Device models made with ABM can be used for most cases,
are much easier to create, and are compatible with PSpice
updates.
276
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
The ABM.OLB part library file
The part library ABM.OLB contains theABM components.
This library contains two sections.
The first section has parts that you can quickly connect to form
control system types of circuits. These components have
names like SUM, GAIN, LAPLACE, and HIPASS.
The second section contains parts that are useful for more
traditional controlled source forms of schematic parts. These
PSpice-equivalent parts have names like EVALUE and
GFREQ and are based on extensions to traditional PSpice E
and G device types.
Implement ABM components by using PSpice primitives;
there is no corresponding ABM.LIB model library. A few
components generate multi-line netlist entries, but most are
implemented as single PSpice E or G device declarations.
See ABM part templates on page 280 for a description of
PSPICETEMPLATE properties and their role in generating
netlist declarations. See Implementation of PSpice-equivalent
parts on page 308 for more information about PSpice E and G
syntax.
PSpice User's Guide
277
Chapter 6
Analog behavioral modeling
Product Version 10.5
Placing and specifying ABM parts
Place and connect ABM parts the same way you place other
parts. After you place an ABM part, you can edit the instance
properties to customize the operational behavior of the part.
This is equivalent to defining an ABM expression describing
how inputs are transformed into outputs. The following
sections describe the rules for specifying ABM expressions.
Net names and device names in ABM expressions
In ABM expressions, refer to signals by name. This is also
considerably more convenient than having to connect a wire
from a pin on an ABM component to a point carrying the
voltage of interest.
If you used an expression such as V(2), then the referenced
net (2 in this case) is interpreted as the name of a local or
global net. A local net is a labeled wire or bus segment in a
hierarchical schematic, or a labeled offpage connector. A
global net is a labeled wire or bus segment at the top level, or
a global connector.
Note: The name of an interface port does not extend to any
connected nets. To refer to a signal originating at an
interface port, connect the port to an offpage connector
of the desired name.
OrCAD Capture recognizes these constructs in ABM
expressions:
V(<net name> )
V(<net name> ,<net name> )
I(<vdevice> )
When one of these is recognized, Capture searches for
<net name> or <vdevice> in the net name space or the
device name space, respectively. Names are searched for first
at the hierarchical level of the part being netlisted. If not found
there, then the set of global names is searched. If the
fragment is not found, then a warning is issued but Capture
still outputs the resulting netlist. When a match is found, the
original fragment is replaced by the fully qualified name of the
net or device.
278
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
For example, suppose we have a hierarchical part U1. Inside
the schematic representing U1 we have an ABM expression
including the term V(Reference). If “Reference” is the name of
a local net, then the fragment written to the netlist will be
translated to V(U1_Reference). If “Reference” is the name of
a global net, the corresponding netlist fragment will be
V(Reference).
Names of voltage sources are treated similarly. For example,
an expression including the term I(Vsense) will be output as
I(V_U1_Vsense) if the voltage source exists locally, and as
I(V_Vsense) if the voltage source exists at the top level.
Forcing the use of a global definition
If a net name exists both at the local hierarchical level and at
the top level, the search mechanism used by Capture will find
the local definition. You can override this, and force Capture to
use the global definition, by prefixing the name with a single
quote (') character.
For example, suppose there is a net called Reference both
inside hierarchical part U1 and at the top level. Then, the ABM
fragment V(Reference) will result in V(U1_Reference) in the
netlist, while the fragment V('Reference) will produce
V(Reference).
PSpice User's Guide
279
Chapter 6
Analog behavioral modeling
Product Version 10.5
ABM part templates
For most ABM parts, a single PSpice “E” or “G” device
declaration is output to the netlist per part instance. The
PSPICETEMPLATE property in these cases is
straightforward. For example the LOG part defines an
expression variant of the E device with its output being the
natural logarithm of the voltage between the input pin and
ground:
E^@REFDES %out 0 VALUE { LOG(V(%in)) }
The fragment E^@REFDES is standard. The “E” specifies a
PSpice A/D controlled voltage source (E device); %in and
%out are the input and output pins, respectively; VALUE is the
keyword specifying the type of ABM device; and the
expression inside the curly braces defines the logarithm of the
input voltage.
Several ABM parts produce more than one primitive
PSpice A/D device per part instance. In this case, the
PSPICETEMPLATE property may be quite complicated. An
example is the DIFFER (differentiator) part. This is
implemented as a capacitor in series with a current sensor
together with an E device which outputs a voltage proportional
to the current through the capacitor.
The template has several unusual features: it gives rise to
three primitives in the PSpice A/D netlist, and it creates a local
node for the connection of the capacitor and its
current-sensing V device.
C^@REFDES %in $$U^@REFDES 1\n
V^@REFDES $$U^@REFDES 0 0v\n
E^@REFDES %out 0 VALUE {@GAIN * I(V^@REFDES)}
Note: For clarity, the template is shown on three lines
although the actual template is a single line.
The fragments C^@REFDES, V^@REFDES, and
E^@REFDES create a uniquely named capacitor, current
sensing V device, and E device, respectively. The fragment
$$U^@REFDES creates a name suitable for use as a local
node. The E device generates an output proportional to the
current through the local V device.
280
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Control system parts
Control system parts have single-pin inputs and outputs. The
reference for input and output voltages is analog ground (0)
from the SOURCE.OLB library. An enhancement to PSpice
means these components can be connected together with no
need for dummy load or input resistors.
Table 6-1 lists the control system parts, grouped by function.
Also listed are characteristic properties that may be set. In the
sections that follow, each part and its properties are described
in more detail.
Table 6-1 Control system parts
Category
Part
Basic
CONST
components
SUM
Limiters
Chebyshev
filters
Description
Properties
constant
VALUE
adder
MULT
multiplier
GAIN
gain block
DIFF
subtracter
LIMIT
hard limiter
GLIMIT
limiter with gain LO, HI, GAIN
SOFTLIM
soft (tanh)
limiter
LO, HI, GAIN
LOPASS
lowpass filter
FP, FS,
RIPPLE,
STOP
HIPASS
highpass filter
FP, FS,
RIPPLE,
STOP
GAIN
LO, HI
BANDPASS bandpass filter F0, F1, F2,
F3, RIPPLE,
STOP
BANDREJ
PSpice User's Guide
band reject
(notch) filter
F0, F1, F2,
F3, RIPPLE,
STOP
281
Chapter 6
Analog behavioral modeling
Product Version 10.5
Table 6-1 Control system parts, continued
Category
Part
Description
Properties
integrator
GAIN, IC
differentiator
GAIN
TABLE
lookup table
ROW1...ROW
5
FTABLE
frequency
lookup table
ROW1...ROW
5
LAPLACE
Laplace
expression
NUM,
DENOM
Integrator
INTEG
and
DIFFER
differentiato
r
Table
look-ups
Laplace
transform
Math
ABS
functions
SQRT
(where ‘x’ is
PWR
the input)
282
|x|
x1/2
|x|EXP
EXP
PWRS
xEXP
EXP
LOG
ln(x)
LOG10
log(x)
EXP
ex
SIN
sin(x)
COS
cos(x)
TAN
tan(x)
ATAN
tan -1 (x)
ARCTAN
tan -1 (x)
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Table 6-1 Control system parts, continued
PSpice User's Guide
Category
Part
Description
Properties
Expression
functions
ABM
no inputs, V out EXP1...EXP4
ABM1
1 input, V out
EXP1...EXP4
ABM2
2 inputs, V out
EXP1...EXP4
ABM3
3 inputs, V out
EXP1...EXP4
ABM/I
no input, I out
EXP1...EXP4
ABM1/I
1 input, I out
EXP1...EXP4
ABM2/I
2 inputs, I out
EXP1...EXP4
ABM3/I
3 inputs, I out
EXP1...EXP4
283
Chapter 6
Analog behavioral modeling
Product Version 10.5
Basic components
The basic components provide fundamental functions and in
many cases, do not require specifying property values. These
parts are described below.
CONST
VALUE
constant value
The CONST part outputs the voltage specified by the VALUE
property. This part provides no inputs and one output.
SUM
The SUM part evaluates the voltages of the two input sources,
adds the two inputs together, then outputs the sum. This part
provides two inputs and one output.
MULT
The MULT part evaluates the voltages of the two input
sources, multiplies the two together, then outputs the product.
This part provides two inputs and one output.
GAIN
GAIN
constant gain value
The GAIN part multiplies the input by the constant specified by
the GAIN property, then outputs the result. This part provides
one input and one output.
DIFF
The DIFF part evaluates the voltage difference between two
inputs, then outputs the result. This part provides two inputs
and one output.
284
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Limiters
The Limiters can be used to restrict an output to values
between a set of specified ranges. These parts are described
below.
LIMIT
HI
LO
upper limit value
lower limit value
The LIMIT part constrains the output voltage to a value
between an upper limit (set with the HI property) and a lower
limit (set with the LO property). This part takes one input and
provides one output.
GLIMIT
HI
LO
GAIN
upper limit value
lower limit value
constant gain value
The GLIMIT part functions as a one-line opamp. The gain is
applied to the input voltage, then the output is constrained to
the limits set by the LO and HI properties. This part takes one
input and provides one output.
SOFTLIMIT
HI
LO
GAIN
A, B, V,
TANH
upper limit value
lower limit value
constant gain value
internal variables used to define the
limiting function
The SOFTLIMIT part provides a limiting function much like the
LIMIT device, except that it uses a continuous curve limiting
function, rather than a discontinuous limiting function. This
part takes one input and provides one output.
PSpice User's Guide
285
Chapter 6
Analog behavioral modeling
Product Version 10.5
Caution
Besides the limiters listed above, the ABM.OLB
consists of a legacy part, HILO. This part is in the
library for backward compatibility and should not
be used in your designs.
Chebyshev filters
The Chebyshev filters allow filtering of the signal based on a
set of frequency characteristics. The output of a Chebyshev
filter depends upon the analysis being performed.
Note: PSpice computes the impulse response of each
Chebyshev filter used in a transient analysis during
circuit read-in. This may require considerable
computing time. A message is displayed on your
screen indicating that the computation is in progress.
For DC and bias point, the output is simply the DC response
of the filter. For AC analysis, the output for each frequency is
the filter response at that frequency. For transient analysis, the
output is then the convolution of the past values of the input
with the impulse response of the filter. These rules follow the
standard method of using Fourier transforms.
Note: To obtain a listing of the filter Laplace coefficients for
each stage, choose Setup from the Analysis menu,
click on Options, and enable LIST in the Options dialog
box.
We recommend looking at one or more of the references cited
in Frequency-domain device models on page 315, as well as
some of the following references on analog filter design:
286
■
Ghavsi, M.S. & Laker, K.R., Modern Filter Design,
Prentice-Hall, 1981.
■
Gregorian, R. & Temes, G., Analog MOS Integrated
Circuits, Wiley-Interscience, 1986.
■
Johnson, David E., Introduction to Filter Theory,
Prentice-Hall, 1976.
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
■
Lindquist, Claude S., Active Network Design with
Signal Filtering Applications, Steward & Sons, 1977.
■
Stephenson, F.W. (ed), RC Active Filter Design
Handbook, Wiley, 1985.
■
Van Valkenburg, M.E., Analog Filter Design, Holt,
Rinehart & Winston, 1982.
■
Williams, A.B., Electronic Filter Design Handbook,
McGraw-Hill, 1981.
Each of the Chebyshev filter parts is described in the following
pages.
LOPASS
FS
FP
RIPPLE
STOP
stop band frequency
pass band frequency
pass band ripple in dB
stop band attenuation in dB
The LOPASS part is characterized by two cutoff frequencies
that delineate the boundaries of the filter pass band and stop
band. The attenuation values, RIPPLE and STOP, define the
maximum allowable attenuation in the pass band, and the
minimum required attenuation in the stop band, respectively.
The LOPASS part provides one input and one output.
Figure 6-1 shows an example of a LOPASS filter device. The
filter provides a pass band cutoff of 800 Hz and a stop band
cutoff of 1.2 kHz. The pass band ripple is 0.1 dB and the
minimum stop band attenuation is 50 dB.
Figure 6-1 LOPASS filter part example
Assuming that the input to the filter is the voltage at net 10 and
output is a voltage between nets 5 and 0, this will produce a
PSpice netlist declaration like this:
PSpice User's Guide
287
Chapter 6
Analog behavioral modeling
Product Version 10.5
ELOWPASS 5 0 CHEBYSHEV {V(10)} LP (800Hz 1.2kHz)
.1dB 50dB
HIPASS
FS
FP
RIPPLE
STOP
stop band frequency
pass band frequency
pass band ripple in dB
stop band attenuation in dB
The HIPASS part is characterized by two cutoff frequencies
that delineate the boundaries of the filter pass band and stop
band. The attenuation values, RIPPLE and STOP, define the
maximum allowable attenuation in the pass band, and the
minimum required attenuation in the stop band, respectively.
The HIPASS part provides one input and one output.
Figure 6-2 shows an example of a HIPASS filter device. This
is a high pass filter with the pass band above 1.2 kHz and the
stop band below 800 Hz.
Figure 6-2 HIPASS filter part example
Again, the pass band ripple is 0.1 dB and the minimum stop
band attenuation is 50 dB. This will produce a PSpice netlist
declaration like this:
EHIGHPASS 5 0 CHEBYSHEV {V(10)} HP (1.2kHz 800Hz)
.1dB 50dB
BANDPASS
RIPPLE pass band ripple in dB
STOP
stop band attenuation in dB
F0, F1, cutoff frequencies
F2, F3
288
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
The BANDPASS part is characterized by four cutoff
frequencies. The attenuation values, RIPPLE and STOP,
define the maximum allowable attenuation in the pass band,
and the minimum required attenuation in the stop band,
respectively. The BANDPASS part provides one input and one
output.
Figure 6-3 shows an example of a BANDPASS filter device.
This is a band pass filter with the pass band between 1.2 kHz
and 2 kHz, and stop bands below 800 Hz and above 3 kHz.
Figure 6-3 BANDPASS filter part example
The pass band ripple is 0.1 dB and the minimum stop band
attenuation is 50 dB. This will produce a PSpice A/D netlist
declaration like this:
EBANDPASS 5 0 CHEBYSHEV
+ {V(10)} BP (800 1.2kHz 2kHz 3kHz) .1dB 50dB
BANDREJ
RIPPLE is the pass band ripple in dB
STOP
is the stop band attenuation in dB
F0, F1, are the cutoff frequencies
F2, F3
The BANDREJ part is characterized by four cutoff
frequencies. The attenuation values, RIPPLE and STOP,
define the maximum allowable attenuation in the pass band,
and the minimum required attenuation in the stop band,
respectively. The BANDREJ part provides one input and one
output.
Figure 6-4 shows an example of a BANDREJ filter device.
This is a band reject (or “notch”) filter with the stop band
PSpice User's Guide
289
Chapter 6
Analog behavioral modeling
Product Version 10.5
between 1.2 kHz and 2 kHz, and pass bands below 800 Hz
and above 3 kHz.
Figure 6-4 BANDREJ filter part example
The pass band ripple is 0.1 dB and the minimum stop band
attenuation is 50 dB. This will produce a PSpice netlist
declaration like this:
EBREJ 5 0 CHEBYSHEV {V(10)} BR (800Hz 1.2kHz 3kHz
2kHz) .1dB 50dB
Integrator and differentiator
The integrator and differentiator parts are described below.
INTEG
IC
GAIN
initial condition of the integrator output
gain value
The INTEG part implements a simple integrator. A current
source/capacitor implementation is used to provide support
for setting the initial condition.
DIFFER
GAIN
gain value
The DIFFER part implements a simple differentiator. A voltage
source/capacitor implementation is used. The DIFFER part
provides one input and one output.
290
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Table look-up parts
TABLE and FTABLE parts provide a lookup table that is used
to correlate an input and an output based on a set of data
points. These parts are described below and on the following
pages.
TABLE
ROWn
is an (input, output) pair; by default, up
to five triplets are allowed where n=1, 2,
3, 4, or 5
If more than five values are required,
the part can be customized through the
part editor. Insert additional row
variables into the template using the
same form as the first five, and add
ROWn properties as needed to the list
of properties.
The TABLE part allows the response to be defined by a table
of one to five values. Each row contains an input and a
corresponding output value. Linear interpolation is performed
between entries.
For values outside the table’s range, the device’s output is a
constant with a value equal to the entry with the smallest (or
largest) input. This characteristic can be used to impose an
upper and lower limit on the output. The TABLE part provides
one input and one output.
PSpice User's Guide
291
Chapter 6
Analog behavioral modeling
Product Version 10.5
FTABLE
ROWn
either an (input frequency,
magnitude, phase) triplet, or an
(input frequency, real part,
imaginary part) triplet describing a
complex value; by default, up to five
triplets are allowed where n=1, 2, 3,
4, or 5
If more than five values are
required, the part can be
customized through the part editor.
Insert additional row variables into
the template using the same form
as the first five, and add ROWn
properties as needed to the list of
properties.
DELAY
group delay increment; defaults to 0
if left blank
R_I
table type; if left blank, the
frequency table is interpreted in the
(input frequency, magnitude,
phase) format; if defined with any
value (such as YES), the table is
interpreted in the (input frequency,
real part, imaginary part) format
MAGUNITS
units for magnitude where the value
can be DB (decibels) or MAG (raw
magnitude); defaults to DB if left
blank
PHASEUNITS
units for phase where the value can
be DEG (degrees) or RAD
(radians); defaults to DEG if left
blank
The FTABLE part is described by a table of frequency
responses in either the magnitude/phase domain (R_I= ) or
complex number domain (R_I=YES). The entire table is read
in and converted to magnitude in dB and phase in degrees.
292
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Interpolation is performed between entries. Magnitude is
interpolated logarithmically; phase is interpolated linearly. For
frequencies outside the table’s range, 0 (zero) magnitude is
used. This characteristic can be used to impose an upper and
lower limit on the output.
The DELAY property increases the group delay of the
frequency table by the specified amount. The delay term is
particularly useful when a frequency table device generates a
non-causality warning message during a transient analysis.
The warning message issues a delay value that can be
assigned to the part’s DELAY property for subsequent runs,
without otherwise altering the table.
The output of the part depends on the analysis being done.
For DC and bias point, the output is the zero frequency
magnitude times the input voltage. For AC analysis, the input
voltage is linearized around the bias point (similar to EVALUE
and GVALUE parts, Modeling mathematical or instantaneous
relationships on page 309). The output for each frequency is
then the input times the gain, times the value of the table at
that frequency.
For transient analysis, the voltage is evaluated at each time
point. The output is then the convolution of the past values
with the impulse response of the frequency response. These
rules follow the standard method of using Fourier transforms.
We recommend looking at one or more of the references cited
in Frequency-domain device models on page 315 for more
information.
Note: The table’s frequencies must be in order from lowest to
highest. The TABLE part provides one input and one
output.
Example
A device, ELOFILT, is used as a frequency filter. The input to
the frequency response is the voltage at net 10. The output is
a voltage across nets 5 and 0. The table describes a low pass
filter with a response of 1 (0 dB) for frequencies below 5
kilohertz and a response of 0.001 (-60 dB) for frequencies
above 6 kilohertz. The phase lags linearly with frequency. This
PSpice User's Guide
293
Chapter 6
Analog behavioral modeling
Product Version 10.5
is the same as a constant time delay. The delay is necessary
so that the impulse response is causal. That is, so that the
impulse response does not have any significant components
before time zero. The FTABLE part in Figure 6-5 could be
used.
Figure 6-5 FTABLE part
This part is characterized by the following properties:
ROW1 = 0Hz
ROW2 = 5kHz
ROW3 = 6kHz
DELAY =
R_I =
MAGUNITS =
PHASEUNITS =
0
0
-60
0
-5760
-6912
Since R_I, MAGUNITS, and PHASEUNITS are undefined,
each table entry is interpreted as containing frequency,
magnitude value in dB, and phase values in degrees. Delay
defaults to 0.
This produces a PSpice netlist declaration like this:
ELOFILT 5 0 FREQ {V(10)}
+0Hz
0 0
+5kHz 0 -5760
+6kHz -60 -6912
Since constant group delay is calculated from the values for a
given table entry as:
group delay = phase / 360 / frequency
An equivalent FTABLE instance could be defined using the
DELAY property. For this example, the group delay is 3.2 msec
(6912 / 360 / 6k = 5760 / 360 / 6k = 3.2m). Equivalent property
assignments are:
ROW1 = 0Hz
ROW2 = 5kHz
294
0
0
0
0
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
ROW3 = 6kHz
DELAY = 3.2ms
R_I =
MAGUNITS =
PHASEUNITS =
-60
0
This produces a PSpice netlist declaration like this:
ELOFILT 5 0 FREQ {V(10)}
+0Hz 0 0
+5kHz 0 0
+6kHz -60 0
+DELAY=3.2ms
PSpice User's Guide
295
Chapter 6
Analog behavioral modeling
Product Version 10.5
Laplace transform part
The LAPLACE part specifies a Laplace transform which is
used to determine an output for each input value.
LAPLACE
NUM
numerator of the Laplace
expression
DENOM
denominator of the Laplace
expression
The LAPLACE part uses a Laplace transform description. The
input to the transform is a voltage. The numerator and
denominator of the Laplace transform function are specified
as properties for the part.
Note: Voltages, currents, and TIME may not appear in a
Laplace transform specification.
The output of the part depends on the type of analysis being
done. For DC and bias point, the output is the zero frequency
gain times the value of the input. The zero frequency gain is
the value of the Laplace transform with s=0. For AC analysis,
the output is then the input times the gain times the value of
the Laplace transform. The value of the Laplace transform at
a frequency is calculated by substituting j·ω for s, where ω is
2π·frequency. For transient analysis, the output is the
convolution of the input waveform with the impulse response
of the transform. These rules follow the standard method of
using Laplace transforms.
Example one
The input to the Laplace transform is the voltage at net 10. The
output is a voltage and is applied between nets 5 and 0. For
DC, the output is simply equal to the input, since the gain at
s=0 is 1. The transform, 1/(1+.001·s), describes a simple,
lossy integrator with a time constant of 1 millisecond. This can
be implemented with an RC pair that has a time constant of 1
millisecond.
296
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
For AC analysis, the gain is found by substituting j·ω for s. This
gives a flat response out to a corner frequency of 1000/(2π) =
159 hertz and a roll-off of 6 dB per octave after 159 Hz. There
is also a phase shift centered around 159 Hz. In other words,
the gain has both a real and an imaginary component. For
transient analysis, the output is the convolution of the input
waveform with the impulse response of 1/(1+.001·s). The
impulse response is a decaying exponential with a time
constant of 1 millisecond. This means that the output is the
“lossy integral” of the input, where the loss has a time constant
of 1 millisecond. The LAPLACE part shown in Figure 6-6 could
be used for this purpose.
Figure 6-6 LAPLACE part
The transfer function is the Laplace transform (1/[1+.001*s]).
This LAPLACE part is characterized by the following
properties:
NUM = 1
DENOM = 1 + .001*s
The gain and phase characteristics are shown in Figure 6-7.
Figure 6-7 Viewing gain and phase characteristics of a
lossy integrator.
PSpice User's Guide
297
Chapter 6
Analog behavioral modeling
Product Version 10.5
This produces a PSpice netlist declaration like this:
ERC
5 0 LAPLACE {V(10)} = {1/(1+.001*s)}
Example two
The input is V(10). The output is a current applied between
nets 5 and 0. The Laplace transform describes a lossy
transmission line. R, L, and C are the resistance, inductance,
and capacitance of the line per unit length.
If R is small, the characteristic impedance of such a line is
Z = ((R + j·ω·L)/(j·ω·C))1/2, the delay per unit length is (L C)1/2,
and the loss in dB per unit length is 23·R/Z. This could be
represented by the device in Figure 6-8.
Figure 6-8 LAPLACE part
The parameters R, L, and C can be defined in a .PARAM
statement contained in a model file. (Refer to the online
PSpice Reference Guide for more information about using
.PARAM statements.) More useful, however, is for R, L, and C
to be arguments passed into a subcircuit. This part has the
following characteristics:
NUM = EXP(-SQRT(C*s*(R+L*s)))
DENOM = 1
This produces a PSpice netlist declaration like this:
GLOSSY 5 0 LAPLACE {V(10)} = {exp(-sqrt(C*s*(R +
L*s)))}
The Laplace transform parts are, however, an inefficient way,
in both computer time and memory, to implement a delay. For
ideal delays we recommend using the transmission line part
instead.
298
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Math functions
The ABM math function parts are shown in Table 6-2. Math
function parts are based on the PSpice “E” device type. Each
provides one or more inputs, and a mathematical function
which is applied to the input. The result is output on the output
net.
Table 6-2 ABM math function parts
For this
device...
Output is the...
ABS
absolute value of the input
SQRT
square root of the input
PWR
result of raising the absolute value of the
input to the power specified by EXP
PWRS
result of raising the (signed) input value to
the power specified by EXP
LOG
LOG of the input
LOG10
LOG10 of the input
EXP
result of e raised to the power specified by
the input value (e x where x is the input)
SIN
sin of the input (where the input is in
radians)
COS
cos of the input (where the input is in
radians)
TAN
tan of the input (where the input is in
radians)
ATAN,
ARCTAN
tan -1 of the input (where the output is in
radians)
ABM expression parts
The expression parts are shown in Table 6-3. These parts can
be customized to perform a variety of functions depending on
your requirements. Each of these parts has a set of four
expression building block properties of the form:
PSpice User's Guide
299
Chapter 6
Analog behavioral modeling
Product Version 10.5
EXPn
where n = 1, 2, 3, or 4.
During netlist generation, the complete expression is formed
by concatenating the building block expressions in numeric
order, thus defining the transfer function. Hence, the first
expression fragment should be assigned to the EXP1
property, the second fragment to EXP2, and so on.
Expression properties can be defined using a combination of
arithmetic operators and input designators. You may use any
of the standard PSpice arithmetic operators (see Table 3-3 on
page 126) within an expression statement. You may also use
the EXPn properties as variables to represent nets or
constants.
Table 6-3 ABM expression parts
Part
Inputs
Output
ABM
none
V
ABM1
1
V
ABM2
2
V
ABM3
3
V
ABM/I
none
I
ABM1/I
1
I
ABM2/I
2
I
ABM3/I
3
I
The following examples illustrate a variety of ABM expression
part applications.
Example one
Suppose you want to set an output voltage on net 4 to 5 volts
times the square root of the voltage between nets 3 and 2. You
could use an ABM2 part (which takes two inputs and provides
300
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
a voltage output) to define a part like the one shown in Figure
6-9.
Figure 6-9 ABM expression part example one.
In this example of an ABM device, the output voltage is set to
5 volts times the square root of the voltage between net 3 and
net 2. The property settings for this part are as follows:
EXP1 = 5V *
EXP2 = SQRT(V(%IN2,%IN1))
This will produce a PSpice netlist declaration like this:
ESQROOT 4 0 VALUE = {5V*SQRT(V(3,2))}
Example two
GPSK is an oscillator for a PSK (Phase Shift Keyed)
modulator. Current is pumped from net 11 through the source
to net 6. Its value is a sine wave with an amplitude of 15 mA
and a frequency of 10 kHz. The voltage at net 3 can shift the
phase of GPSK by 1 radian/volt. Note the use of the TIME
parameter in the EXP2 expression. This is the PSpice A/D
internal sweep variable used in transient analysis. For any
analysis other than transient, TIME = 0. This could be
represented with an ABM1/I part (single input, current output)
like the one shown in Figure 6-10.
Figure 6-10 ABM expression part example two.
PSpice User's Guide
301
Chapter 6
Analog behavioral modeling
Product Version 10.5
This part is characterized by the following properties:
EXP1 = 15ma * SIN(
EXP2 = 6.28*10kHz*TIME
EXP3 = + V(%IN))
This produces a PSpice netlist declaration like this:
GPSK
11 6 VALUE =
{15MA*SIN(6.28*10kHz*TIME+V(3))}
Example three
A device, EPWR, computes the instantaneous power by
multiplying the voltage across nets 5 and 4 by the current
through VSENSE. Sources are controlled by expressions
which may contain voltages or currents or both. The ABM2
part (two inputs, voltage output) in Figure 6-11 could represent
this.
Figure 6-11 ABM expression part example three.
This part is characterized by the following properties:
EXP1 = V(%IN2,%IN1) *
EXP2 = I(VSENSE)
This produces a PSpice netlist declaration like this:
EPWR
3 0 VALUE = {V(5,4)*I(VSENSE)}
Example four
The output of a component, GRATIO, is a current whose value
(in amps) is equal to the ratio of the voltages at nets 13 and 2.
If V(2) = 0, the output depends upon V(13) as follows:
if V(13) = 0, output = 0
if V(13) > 0, output = MAXREAL
if V(13) < 0, output = -MAXREAL
302
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
where MAXREAL is a PSpice internal constant representing a
very large number (on the order of 1e30). In general, the result
of evaluating an expression is limited to MAXREAL. This is
modeled with an ABM2/I (two input, current output) part like
this one in 6-12.
Figure 6-12 ABM expression part example four.
This part is characterized by the following properties:
EXP1 = V(%IN2)/V(%IN1)
Note that output of GRATIO can be used as part of the
controlling function. This produces a PSpice netlist
declaration like this:
GRATIO 2 3 VALUE = {V(13)/V(2)}
Note: Letting a current approach 1e30 will almost certainly
cause convergence problems. To avoid this, use the
limit function on the ratio to keep the current within
reasonable limits.
An instantaneous device example: modeling a triode
This section provides an example of using various ABM parts
to model a triode vacuum tube. The schematic of the triode
subcircuit is shown in Figure 6-13.
PSpice User's Guide
303
Chapter 6
Analog behavioral modeling
Product Version 10.5
Figure 6-13 Triode circuit.
Assumptions: In its main operating region, the triode’s current
is proportional to the 3/2 power of a linear combination of the
grid and anode voltages:
ianode = k0*(vg + k1*va)1.5
For a typical triode, k0 = 200e-6 and k1 = 0.12.
Looking at the upper left-hand portion of the schematic, notice
the a general-purpose ABM part used to take the input
voltages from anode, grid, and cathode. Assume the following
associations:
■
V(anode) is associated with V(%IN1)
■
V(grid) is associated with V(%IN2)
■
V(cathode) is associated with V(%IN3)
The expression property EXP1 then represents V(grid,
cathode) and the expression property EXP2 represents
0.12[V(anode, cathode)]. When the template substitution is
performed, the resulting VALUE is equivalent to the following:
V = V(grid, cathode) + 0.12*V(anode, cathode)
The part would be defined with the following characteristics:
EXP1 = V(%IN2,%IN3)+
EXP2 = 0.12*V(%IN1,%IN3)
This works for the main operating region but does not model
the case in which the current stays 0 when combined grid and
anode voltages go negative. We can accommodate that
situation as follows by adding the LIMIT part with the following
characteristics:
HI = 1E3
LO = 0
This part instance, LIMIT1, converts all negative values of
vg+.12*va to 0 and leaves all positive values (up to 1 kV) alone.
For a more realistic model, we could have used TABLE to
correctly model how the tube turns off at 0 or at small negative
grid voltages.
304
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
We also need to make sure that the current becomes zero
when the anode alone goes negative. To do this, we can use
a DIFF device, (immediately below the ABM3 device) to
monitor the difference between V(anode) and V(cathode), and
output the difference to the TABLE part. The table translates
all values at or below zero to zero, and all values greater than
or equal to 30 to one. All values between 0 and 30 are linearly
interpolated. The properties for the TABLE part are as follows:
ROW1 = 00
ROW2 = 301
The TABLE part is a simple one, and ensures that only a zero
value is output to the multiplier for negative anode voltages.
The output from the TABLE part and the LIMIT part are
combined at the MULT multiplier part. The output of the MULT
part is the product of the two input voltages. This value is then
raised to the 3/2 or 1.5 power using the PWR part. The
exponential property of the PWR part is defined as follows:
EXP = 1.5
The last major component is an ABM expression component
to take an input voltage and convert it into a current. The
relevant ABM1/I part property looks like this:
EXP1 = 200E-6 * V(%IN)
A final step in the model is to add device parasitics. For
example, a resistor can be used to give a finite output
impedance. Capacitances between the grid, cathode, and
anode are also needed. The lower part of the schematic in
Figure 6-13 shows a possible method for incorporating these
effects. To complete the example, one could add a circuit
PSpice User's Guide
305
Chapter 6
Analog behavioral modeling
Product Version 10.5
which produces the family of I-V curves (shown in Figure
6-14).
Figure 6-14 Triode subcircuit producing a family of I-V
curves.
306
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
PSpice-equivalent parts
PSpice-equivalent parts respond to a differential input and
have double-ended output. These parts reflect the structure of
PSpice E and G devices, thus having two pins for each
controlling input and the output in the part. Table 6-4
summarizes the PSpice-equivalent parts available in the part
library.
Table 6-4 PSpice-equivalent parts
Category
Part
Mathematical EVALUE
expression
GVALUE
ESUM
Description
Properties
general purpose EXPR
special purpose
(none)
GSUM
EMULT
GMULT
Table look-up ETABLE
GTABLE
Frequency
table look-up
EFREQ
Laplace
transform
ELAPLACE
GFREQ
GLAPLACE
general purpose EXPR
TABLE
general purpose EXPR
TABLE
general purpose EXPR
XFORM
PSpice-equivalent ABM parts can be classified as either E or
G device types. The E part type provides a voltage output, and
the G device type provides a current output.
The device’s transfer function can contain any mixture of
voltages and currents as inputs. Hence, there is no longer a
division between voltage-controlled and current-controlled
parts. Rather the part type is dictated only by the output
requirements. If a voltage output is required, use an E part
type. If a current output is necessary, use a G part type.
PSpice User's Guide
307
Chapter 6
Analog behavioral modeling
Product Version 10.5
Note: There are no equivalent “F” or “H” part types in the part
library because PSpice “F” and “H” devices do not
support the ABM extensions.
Each E or G part type in the ABM.OLB part file is defined by a
template that provides the specifics of the transfer function.
Other properties in the model definition can be edited to
customize the transfer function. By default, the template
cannot be modified directly choosing Properties from the Edit
menu in Capture. Rather, the values for other properties (such
as the expressions used in the template) are usually edited,
then these values are substituted into the template. However,
the part editor can be used to modify the template or
designate the template as modifiable from within Capture.
This way, custom parts can be created for special-purpose
application.
Implementation of PSpice-equivalent parts
Although you generally use Capture to place and specify
PSpice-equivalent ABM parts, it is useful to know the PSpice
command syntax for “E” and “G” devices. This is especially
true when creating custom ABM parts since part templates
must adhere to PSpice syntax.
The general forms for PSpice “E” and “G” extensions are:
E <name> <connecting nodes> <ABM keyword>
<ABM function>
G <name> <connecting nodes> <ABM keyword>
<ABM function>
where
<name>
is the device name appended to the E or G
device type character
<connecting specifies the <(+ node name, - node
nodes>
name)> pair between which the device is
connected
308
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
<ABM
keyword>
<ABM
function>
specifies the form of the transfer function to
be used, as one of:
VALUE
arithmetic expression
TABLE
lookup table
LAPLACE
Laplace transform
FREQ
frequency response table
CHEBYSHEV Chebyshev filter
characteristics
specifies the transfer function as a formula or
lookup table as required by the specified
<ABM keyword>
Refer to the online PSpice Reference Guide for detailed
information.
Modeling mathematical or instantaneous relationships
The instantaneous models (using VALUE and TABLE
extensions to PSpice “E” and “G” devices in the part
templates) enforce a direct response to the input at each
moment in time. For example, the output might be equal to the
square root of the input at every point in time. Such a device
has no memory, or, a flat frequency response. These
techniques can be used to model both linear and nonlinear
responses.
Note: For AC analysis, a nonlinear device is first linearized
around the bias point, and then the linear equivalent is
used.
EVALUE and GVALUE parts
The EVALUE and GVALUE parts allow an instantaneous
transfer function to be written as a mathematical expression in
standard notation. These parts take the input signal, perform
the function specified by the EXPR property on the signal, and
output the result on the output pins.
In controlled sources, EXPR may contain constants and
parameters as well as voltages, currents, or time. Voltages
may be either the voltage at a net, such as V(5), or the voltage
across two nets, such as V(4,5). Currents must be the current
PSpice User's Guide
309
Chapter 6
Analog behavioral modeling
Product Version 10.5
through a voltage source (V device), for example, I(VSENSE).
Voltage sources with a value of 0 are handy for sensing
current for use in these expressions.
Functions may be used in expressions, along with arithmetic
operators (+, -, *, and /) and parentheses. Available built-in
functions are summarized in Table 3-4 on page 126.
The EVALUE and GVALUE parts are defined, in part, by the
following properties (default values are shown):
EVALUE
EXPR
V(%IN+, %IN-)
GVALUE
EXPR
V(%IN+, %IN-)
Sources are controlled by expressions which may contain
voltages, currents, or both. The following examples illustrate
customized EVALUE and GVALUE parts.
Example 1
In the example of an EVALUE device shown in Figure 6-15,
the output voltage is set to 5 volts times the square root of the
voltage between pins %IN+ and %IN-.
Figure 6-15 EVALUE part example.
The property settings for this device are as follows:
EXPR = 5v * SQRT(V(%IN+,%IN-))
310
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Example 2
Consider the device in Figure 6-16. This device could be used
as an oscillator for a PSK (Phase Shift Keyed) modulator.
Figure 6-16 GVALUE part example.
A current through a source is a sine wave with an amplitude of
15 mA and a frequency of 10 kHz. The voltage at the input pin
can shift the phase by 1 radian/volt. Note the use of the TIME
parameter in this expression. This is the PSpice internal
sweep variable used in transient analyses. For any analysis
other than transient, TIME = 0. The relevant property settings
for this device are shown below:
EXPR = 15ma*SIN(6.28*10kHz*TIME+V(%IN+,%IN-))
EMULT, GMULT, ESUM, and GSUM
The EMULT and GMULT parts provide output which is based
on the product of two input sources. The ESUM and GSUM
parts provide output which is based on the sum of two input
sources. The complete transfer function may also include
other mathematical expressions.
Example 1
Consider the device in Figure 6-17. This device computes the
instantaneous power through resistor VSENSE by multiplying
PSpice User's Guide
311
Chapter 6
Analog behavioral modeling
Product Version 10.5
the current through VSENSE (converted to voltage by H1) by
the voltage across VSENSE.
Figure 6-17 EMULT part example.
This device’s behavior is built-in to the PSPICETEMPLATE
property as follows (appears on one line):
TEMPLATE=E^@REFDES %OUT+ %OUT- VALUE
{V(%IN1+,%IN1-)
*V(%IN2+,%IN2-)}
You can use the part editor to change the characteristics of the
template to accommodate additional mathematical functions,
or to change the nature of the transfer function itself. For
example, you may want to create a voltage divider, rather than
a multiplier. This is illustrated in the following example.
Example 2
Consider the device in Figure 6-18.
Figure 6-18 GMULT part example.
With this device, the output is a current is equal to the ratio of
the voltages at input pins 1 and input pins 2. If V(%IN2+,
312
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
%IN2-) = 0, the output depends upon V(%IN1+, %IN1-) as
follows:
if V(%IN1+, %IN1-) = 0, output = 0
if V(%IN1+, %IN1-) > 0, output = MAXREAL
if V(%IN1+, %IN1-) < 0, output = -MAXREAL
where MAXREAL is a PSpice internal constant representing a
very large number (on the order of 1e30). In general, the result
of evaluating an expression is limited to MAXREAL. Note that
the output of the part can also be used as part of the
controlling function.
To create this device, you would first make a new part, GDIV,
based on the GMULT part. Edit the GDIV template to divide
the two input values rather than multiply them.
Lookup tables (ETABLE and GTABLE)
The ETABLE and GTABLE parts use a transfer function
described by a table. These device models are well suited for
use with measured data.
The ETABLE and GTABLE parts are defined in part by the
following properties (default values are shown):
ETABLE
TABLE
EXPR
(-15, -15), (15,15)
V(%IN+, %IN-)
GTABLE
TABLE
EXPR
(-15, -15), (15,15)
V(%IN+, %IN-)
First, EXPR is evaluated, and that value is used to look up an
entry in the table. EXPR is a function of the input (current or
voltage) and follows the same rules as for VALUE
expressions.
The table consists of pairs of values, the first of which is an
input, and the second of which is the corresponding output.
Linear interpolation is performed between entries. For values
of EXPR outside the table’s range, the device’s output is a
PSpice User's Guide
313
Chapter 6
Analog behavioral modeling
Product Version 10.5
constant with a value equal to the entry with the smallest (or
largest) input. This characteristic can be used to impose an
upper and lower limit on the output.
An example of a table declaration (using the TABLE property)
would be the following:
TABLE =
+ (0, 0) (.02, 2.690E-03) (.04, 4.102E-03) (.06,
4.621E-03)
+ (.08, 4.460E-03) (.10, 3.860E-03) (.12, 3.079E-03)
(.14,
+ 2.327E-03)
+ (.16, 1.726E-03) (.18, 1.308E-03) (.20, 1.042E-03)
(.22,
+ 8.734E-04)
+ (.24, 7.544E-04) (.26, 6.566E-04) (.28, 5.718E-04)
(.30,
+ 5.013E-04)
+ (.32, 4.464E-04) (.34, 4.053E-04) (.36, 3.781E-04)
(.38,
+ 3.744E-04)
+ (.40, 4.127E-04) (.42, 5.053E-04) (.44, 6.380E-04)
(.46,
+ 7.935E-04)
+ (.48, 1.139E-03) (.50, 2.605E-03) (.52, 8.259E-03)
(.54,
+ 2.609E-02)
+ (.56, 7.418E-02) (.58, 1.895E-01) (.60, 4.426E-01)
314
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Frequency-domain device models
Frequency-domain models (ELAPLACE, GLAPLACE,
EFREQ, and GFREQ) are characterized by output that
depends on the current input as well as the input history. The
relationship is therefore non-instantaneous. For example, the
output may be equal to the integral of the input over time. In
other words, the response depends upon frequency.
During AC analysis, the frequency response determines the
complex gain at each frequency. During DC analysis and bias
point calculation, the gain is the zero-frequency response.
During transient analysis, the output of the device is the
convolution of the input and the impulse response of the
device.
Moving back and forth between the time and
frequency-domains can cause surprising results. Often the
results are quite different than what one would intuitively
expect. For this reason, we strongly recommend familiarity
with a reference on Fourier and Laplace transforms. A good
one is:
■
R. Bracewell, The Fourier Transform and Its Applications,
McGraw-Hill, Revised Second Edition (1986)
We also recommend familiarity with the use of transforms in
analyzing linear systems. Some references on this subject:
■
W. H. Chen, The Analysis of Linear Systems,
McGraw-Hill (1962)
■
J. A. Aseltine, Transform Method in Linear System
Analysis, McGraw-Hill (1958)
Laplace transforms (LAPLACE)
The ELAPLACE and GLAPLACE parts allow a transfer
function to be described by a Laplace transform function. The
ELAPLACE and GLAPLACE parts are defined, in part, by the
following properties (default values are shown):
ELAPLACE
PSpice User's Guide
315
Chapter 6
Analog behavioral modeling
Product Version 10.5
EXPR
XFORM
V(%IN+, %IN-)
1/s
GLAPLACE
EXPR
XFORM
V(%IN+, %IN-)
1/s
The LAPLACE parts use a Laplace transform description. The
input to the transform is the value of EXPR, where EXPR
follows the same rules as for VALUE expressions (see
EVALUE and GVALUE parts on page 309). XFORM is an
expression in the Laplace variable, s. It follows the rules for
standard expressions as described for VALUE expressions
with the addition of the s variable.
Note: Voltages, currents, and TIME cannot appear in a
Laplace transform.
The output of the device depends on the type of analysis
being done. For DC and bias point, the output is simply the
zero frequency gain times the value of EXPR. The zero
frequency gain is the value of XFORM with s = 0. For AC
analysis, EXPR is linearized around the bias point (similar to
the VALUE parts). The output is then the input times the gain
of EXPR times the value of XFORM. The value of XFORM at
a frequency is calculated by substituting j·w for s, where w is
2p·frequency. For transient analysis, the value of EXPR is
evaluated at each time point. The output is then the
convolution of the past values of EXPR with the impulse
response of XFORM. These rules follow the standard method
of using Laplace transforms. We recommend looking at one or
more of the references cited in Frequency-domain device
models on page 315 for more information.
Example
The input to the Laplace transform is the voltage across the
input pins, or V(%IN+, %IN-). The EXPR property may be
edited to include constants or functions, as with other parts.
The transform, 1/(1+.001·s), describes a simple, lossy
integrator with a time constant of 1 millisecond. This can be
implemented with an RC pair that has a time constant of 1
millisecond.
316
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
Using the part editor, you would define the XFORM and EXPR
properties as follows:
XFORM = 1/(1+.001*s)
EXPR = V(%IN+, %IN-)
The default template remains (appears on one line):
TEMPLATE= E^@REFDES %OUT+ %OUT- LAPLACE {@EXPR}=
(@XFORM)
After netlist substitution of the template, the resulting transfer
function would become:
V(%OUT+, %OUT-) = LAPLACE {V(%IN+, %IN-)}=
(1/1+.001*s))
The output is a voltage and is applied between pins %OUT+
and %OUT-. For DC, the output is simply equal to the input,
since the gain at s = 0 is 1.
For AC analysis, the gain is found by substituting j·ω for s. This
gives a flat response out to a corner frequency of 1000/(2π) =
159 Hz and a roll-off of 6 dB per octave after 159 Hz. There is
also a phase shift centered around 159 Hz. In other words, the
gain has both a real and an imaginary component. The gain
and phase characteristic is the same as that shown for the
equivalent control system part example using the LAPLACE
part (see Figure 6-7 on page 297).
For transient analysis, the output is the convolution of the input
waveform with the impulse response of 1/(1+.001·s). The
impulse response is a decaying exponential with a time
constant of 1 millisecond. This means that the output is the
“lossy integral” of the input, where the loss has a time constant
of 1 millisecond.
This will produce a PSpice A/D netlist declaration similar to:
ERC 5 0 LAPLACE {V(10)} = {1/(1+.001*s)}
Frequency response tables (EFREQ and GFREQ)
The EFREQ and GFREQ parts are described by a table of
frequency responses in either the magnitude/phase domain or
complex number domain. The entire table is read in and
converted to magnitude in dB and phase in degrees.
Interpolation is performed between entries. Phase is
PSpice User's Guide
317
Chapter 6
Analog behavioral modeling
Product Version 10.5
interpolated linearly; magnitude is interpolated logarithmically.
For frequencies outside the table’s range, 0 (zero) magnitude
is used.
EFREQ and GFREQ properties are defined as follows:
EXPR
TABLE
DELAY
R_I
MAGUNITS
PHASEUNITS
value used for table lookup; defaults to
V(%IN+, %IN-) if left blank.
series of either (input frequency,
magnitude, phase) triplets, or (input
frequency, real part, imaginary part)
triplets describing a complex value;
defaults to (0,0,0) (1Meg,-10,90) if left
blank.
group delay increment; defaults to 0 if left
blank.
table type; if left blank, the frequency
table is interpreted in the (input
frequency, magnitude, phase) format; if
defined with any value (such as YES), the
table is interpreted in the (input
frequency, real part, imaginary part)
format.
units for magnitude where the value can
be DB (decibels) or MAG (raw
magnitude); defaults to DB if left blank.
units for phase where the value can be
DEG (degrees) or RAD (radians);
defaults to DEG if left blank.
The DELAY property increases the group delay of the
frequency table by the specified amount. The delay term is
particularly useful when an EFREQ or GFREQ device
generates a non-causality warning message during a
transient analysis. The warning message issues a delay value
that can be assigned to the part’s DELAY property for
subsequent runs, without otherwise altering the table.
The output of the device depends on the analysis being done.
For DC and bias point, the output is simply the zero frequency
magnitude times the value of EXPR. For AC analysis, EXPR
is linearized around the bias point (similar to EVALUE and
GVALUE parts). The output for each frequency is then the
318
PSpice User's Guide
Product Version 10.5
The ABM.OLB part library file
input times the gain of EXPR times the value of the table at
that frequency. For transient analysis, the value of EXPR is
evaluated at each time point. The output is then the
convolution of the past values of EXPR with the impulse
response of the frequency response. These rules follow the
standard method of using Fourier transforms. We recommend
looking at one or more of the references cited in
Frequency-domain device models on page 315 for more
information.
Note: The table’s frequencies must be in order from lowest to
highest.
Figure 6-19 shows an EFREQ device used as a low pass filter.
Figure 6-19 EFREQ part example.
The input to the frequency response is the voltage across the
input pins. The table describes a low pass filter with a
response of 1 (0 dB) for frequencies below 5 kilohertz and a
response of .001 (-60 dB) for frequencies above 6 kilohertz.
The output is a voltage across the output pins.
This part is defined by the following properties:
TABLE = (0, 0, 0) (5kHz, 0, -5760) (6kHz, -60, -6912)
DELAY =
R_I =
MAGUNITS =
PHASEUNITS =
Since R_I, MAGUNITS, and PHASEUNITS are undefined,
each table entry is interpreted as containing frequency,
magnitude value in dB, and phase values in degrees. Delay
defaults to 0.
The phase lags linearly with frequency meaning that this table
exhibits a constant time (group) delay. The delay is necessary
so that the impulse response is causal. That is, so that the
PSpice User's Guide
319
Chapter 6
Analog behavioral modeling
Product Version 10.5
impulse response does not have any significant components
before time zero.
The constant group delay is calculated from the values for a
given table entry as follows:
group delay = phase / 360 / frequency
For this example, the group delay is 3.2 msec
(6912 / 360 / 6k = 5760 / 360 / 6k = 3.2m). An alternative
specification for this table could be:
TABLE = (0, 0, 0) (5kHz, 0, 0) (6kHz, -60, 0)
DELAY = 3.2ms
R_I =
MAGUNITS =
PHASEUNITS =
This produces a PSpice netlist declaration like this:
ELOWPASS 5 0 FREQ {V(10)} = (0,0,0) (5kHz,0,0)
(6kHz-60,0)
+ DELAY = 3.2ms
Cautions and recommendations for simulation and
analysis
Instantaneous device modeling
During AC analysis, nonlinear transfer functions are handled
the same way as other nonlinear parts: each function is
linearized around the bias point and the resulting small-signal
equivalent is used.
Consider the voltage multiplier (mixer) shown in Figure 6-20.
Figure 6-20 Voltage multiplier circuit (mixer).
320
PSpice User's Guide
Product Version 10.5
Cautions and recommendations for simulation and analysis
This circuit has the following characteristics:
Vin1:
Vin2:
DC=0v AC=1v
DC=0v AC=1v
where the output on net 3 is V(1)*V(2).
During AC analysis, V(3) = 0 due to the 0 volts bias point
voltage on nets 1, 2, and 3. The small-signal equivalent
therefore has 0 gain (the derivative of V(1)*V(2) with respect
to both V(1) and V(2) is 0 when V(1)=V(2)=0). So, the output
of the mixer during AC analysis will be 0 regardless of the AC
values of V(1) and V(2).
Another way of looking at this is that a mixer is a nonlinear
device and AC analysis is a linear analysis. The output of the
mixer has 0 amplitude at the fundamental. (Output is nonzero
at DC and twice the input frequency, but these are not
included in a linear analysis.)
If you need to analyze nonlinear functions, such as a mixer,
use transient analysis. Transient analysis solves the full,
nonlinear circuit equations. It also allows you to use input
waveforms with different frequencies (for example, VIN1 could
be 90 MHz and VIN2 could be 89.8 MHz). AC analysis does
not have this flexibility, but in return it uses much less
computer time.
Frequency-domain parts
Some caution is in order when moving between frequency and
time domains. This section discusses several points that are
involved in the implementation of frequency-domain parts.
These discussions all involve the transient analysis, since
both the DC and AC analyses are straightforward.
The first point is that there are limits on the maximum values
and on the resolution of both time and frequency. These are
related: the frequency resolution is the inverse of the
maximum time and vice versa. The maximum time is the
length of the transient analysis, TSTOP. Therefore, the
frequency resolution is 1/TSTOP.
PSpice User's Guide
321
Chapter 6
Analog behavioral modeling
Product Version 10.5
Laplace transforms
For Laplace transforms, PSpice starts off with initial bounds
on the frequency resolution and the maximum frequency
determined by the transient analysis parameters as follows.
The frequency resolution is initially set below the theoretical
limit to (.25/TSTOP) and is then made as large as possible
without inducing sampling errors. The maximum frequency
has an initial upper bound of (1/(RELTOL*TMAX)), where
TMAX is the transient analysis Step Ceiling value, and
RELTOL is the relative accuracy of all calculated voltages and
currents. If a Step Ceiling value is not specified, PSpice uses
the Transient Analysis Print Step, TSTEP, instead.
Note: TSTOP, TMAX, and TSTEP values are configured
using Transient on the Setup menu. The RELTOL
property is set using Options on the Setup menu.
PSpice then attempts to reduce the maximum frequency by
searching for the frequency at which the response has fallen
to RELTOL times the maximum response. For instance, for the
transform:
1/(1+s)
the maximum response, 1.0, is at s = j·ω = 0 (DC). The cutoff
frequency used when RELTOL=.001, is approximately
1000/(2π) = 159 Hz. At 159 Hz, the response is down to .001
(down by 60 db). Since some transforms do not have such a
limit, there is also a limit of 10/RELTOL times the frequency
resolution, or 10/(RELTOL·TSTOP). For example, consider
the transform:
e -0.001·s
This is an ideal delay of 1 millisecond and has no frequency
cutoff. If TSTOP = 10 milliseconds and RELTOL=.001, then
PSpice imposes a frequency cutoff of 10 MHz. Since the time
resolution is the inverse of the maximum frequency, this is
equivalent to saying that the delay cannot resolve changes in
the input at a rate faster than .1 microseconds. In general, the
time resolution will be limited to RELTOL·TSTOP/10.
A final computational consideration for Laplace parts is that
the impulse response is determined by means of an FFT on
322
PSpice User's Guide
Product Version 10.5
Cautions and recommendations for simulation and analysis
the Laplace expression. The FFT is limited to 8192 points to
keep it tractable, and this places an additional limit on the
maximum frequency, which may not be greater than 8192
times the frequency resolution.
If your circuit contains many Laplace parts which can be
combined into a more complex single device, it is generally
preferable to do this. This saves computation and memory
since there are fewer impulse responses. It also reduces the
number of opportunities for numerical artifacts that might
reduce the accuracy of your transient analyses.
Laplace transforms can contain poles in the left half-plane.
Such poles will cause an impulse response that increases with
time instead of decaying. Since the transient analysis is
always for a finite time span, PSpice does not have a problem
calculating the transient (or DC) response. However, such
poles will make the actual device oscillate.
Non-causality and Laplace transforms
PSpice applies an inverse FFT to the Laplace expression to
obtain an impulse response, and then convolves the impulse
response with the dependent source input to obtain the
output. Some common impulse responses are inherently
non-causal. This means that the convolution must be applied
to both past and future samples of the input in order to
properly represent the inverse of the Laplace expression.
For example, the expression {S} corresponds to differentiation
in the time domain. The impulse response for {S} is an impulse
pair separated by an infinitesimal distance in time. The
impulses have opposite signs, and are situated one in the
infinitesimal past, the other in the infinitesimal future. In other
words, convolution with this corresponds to applying a
finite-divided difference in the time domain.
The problem with this for PSpice is that the simulator only has
the present and past values of the simulated input, so it can
only apply half of the impulse pair during convolution. This will
obviously not result in time-domain differentiation. PSpice can
detect, but not fix this condition, and issues a non-causality
warning message when it occurs. The message tells what
PSpice User's Guide
323
Chapter 6
Analog behavioral modeling
Product Version 10.5
percentage of the impulse response is non-causal, and how
much delay would need to be added to slide the non-causal
part into a causal region. {S} is theoretically 50% non-causal.
Non-causality on the order of 1% or less is usually not critical
to the simulation results.
You can delay {S} to keep it causal, but the separation
between the impulses is infinitesimal. This means that a very
small time step is needed. For this reason, it is usually better
to use a macromodel to implement differentiation.
Here are some guidelines:
■
In the case of a Laplace device (ELAPLACE), multiply the
Laplace expression by e to the
(-s ∗ <the suggested delay>).
■
In the case of a frequency table (EFREQ or GFREQ), do
either of the following:
❑
Specify the table with
DELAY=<the suggested delay>.
❑
Compute the delay by adding a phase shift.
Chebyshev filters
All of the considerations given above for Laplace parts also
apply to Chebyshev filter parts. However, PSpice A/D also
attempts to deal directly with inaccuracies due to sampling by
applying Nyquist criteria based on the highest filter cutoff
frequency. This is done by checking the value of TMAX. If
TMAX is not specified it is assigned a value, or if it is specified,
it may be reduced.
For low pass and band pass filters, TMAX is set to (0.5/FS),
where FS is the stop band cutoff in the case of a low pass filter,
or the upper stop band cutoff in the case of a band pass filter.
For high pass and band reject filters, there is no clear way to
apply the Nyquist criterion directly, so an additional factor of
two is thrown in as a safety margin. Thus, TMAX is set to
(0.25/FP), where FP is the pass band cutoff for the high pass
case or the upper pass band cutoff for the band reject case. It
may be necessary to set TMAX to something smaller if the
324
PSpice User's Guide
Product Version 10.5
Cautions and recommendations for simulation and analysis
filter input has significant frequency content above these
limits.
Frequency tables
For frequency response tables, the maximum frequency is
twice the highest value. It will be reduced to
10/(RELTOL⋅TSTOP) or 8192 times the frequency resolution
if either value is smaller.
The frequency resolution for frequency response tables is
taken to be either the smallest frequency increment in the
table or the fastest rate of phase change, whichever is least.
PSpice then checks to see if it can be loosened without
inducing sampling errors.
Trading off computer resources for accuracy
There is a significant trade-off between accuracy and
computation time for parts modeled in the frequency domain.
The amount of computer time and memory scale
approximately inversely to RELTOL. Therefore, if you can use
RELTOL=.01 instead of the default .001, you will be ahead.
However, this will not adversely affect the impulse response.
You may also wish to vary TMAX and TSTOP, since these also
come into play.
Since the trade-off issues are fairly complex, it is advisable to
first simulate a small test circuit containing only the
frequency-domain device, and then after proper validation,
proceed to incorporate it in your larger design. The PSpice
defaults will be appropriate most of the time if accuracy is your
main concern, but it is still worth checking.
Note: Do not set RELTOL to a value above 0.01. This can
seriously compromise the accuracy of your simulation.
PSpice User's Guide
325
Chapter 6
Analog behavioral modeling
Product Version 10.5
Basic controlled sources
As with basic SPICE, PSpice has basic controlled sources
derived from the standard SPICE E, F, G, and H devices. Table
6-5 summarizes the linear controlled source types provided in
the standard part library.
Table 6-5 Basic controlled sources in ANALOG.OLB
Device type
Part name
Controlled Voltage Source
E
(PSpice A/D E device)
Current-Controlled Current Source
F
(PSpice A/D F device)
Controlled Current Source
G
(PSpice A/D G device)
Current-Controlled Voltage Source
H
(PSpice A/D H device)
Creating custom ABM parts
Create a custom part when you need a controlled source that
is not provided in the special purpose set or that is more
elaborate than you can build with the general purpose parts
(with multiple controlling inputs, for example). Refer to your
OrCAD Capture User’s Guide for a description of how to
create a custom part.
The transfer function can be built into the part two different
ways:
■
directly in the PSPICETEMPLATE definition.
■
by defining the part’s EXPR and related properties (if
any).
The PSpice syntax for declaring E and G devices can help you
form a PSPICETEMPLATE definition. Refer to the online
326
PSpice User's Guide
Product Version 10.5
Cautions and recommendations for simulation and analysis
PSpice Reference Guide for more information about E and
G devices.
PSpice User's Guide
327
Chapter 6
328
Analog behavioral modeling
Product Version 10.5
PSpice User's Guide
Digital device modeling
7
Chapter overview
This chapter provides information about digital modeling, and
includes the following sections:
■
Introduction on page 330
■
Functional behavior on page 331
■
Timing characteristics on page 339
■
Input/Output characteristics on page 346
■
Creating a digital model using the PINDLY and
LOGICEXP primitives on page 358
Note: This entire chapter describes features that are not
included in PSpice.
PSpice User's Guide
329
Chapter 7
Digital device modeling
Product Version 10.5
Introduction
The standard part libraries contain a comprehensive set of
digital parts in many different technologies. Each digital part is
described electrically by a digital device model in the form of
a subcircuit definition stored in a model library. The
corresponding subcircuit name is defined by the part’s
MODEL attribute value. Other attributes—MNTYMXDLY,
IO_LEVEL, and the PSPICEDEFAULTNET set—are passed
to the subcircuit, thus providing a high-level means for
influencing the behavior of the digital device model.
Generally, the digital parts provided in the part libraries are
satisfactory for most circuit designs. However, if your design
requires digital parts that are not already provided in the
PSpice part and model libraries, you need to define digital
device models corresponding to the new digital parts.
A complete digital device model has three main
characteristics:
■
Functional behavior: described by the gate-level and
behavioral digital primitives comprising the subcircuit.
■
I/O behavior: described by the I/O model, interface
subcircuits, and power supplies related to a logic family.
■
Timing behavior: described by one or more timing
models, pin-to-pin delay primitives, or constraint checker
primitives.
These characteristics are described in this chapter with a
running example demonstrating the use of gate-level
primitives.
330
PSpice User's Guide
Product Version 10.5
Chapter overview
Functional behavior
A digital device model’s functional behavior is defined by one
or more interconnected digital primitives. Typically, a logic
diagram in a data book can be implemented directly using the
primitives provided by PSpice A/D. The table below provides a
summary of the digital primitives.
Table 7-1 Digital primitives summary
Type
Description
Standard gates
PSpice User's Guide
BUF
buffer
INV
inverter
AND
AND gate
NAND
NAND gate
OR
OR gate
NOR
NOR gate
XOR
exclusive OR gate
NXOR
exclusive NOR gate
BUFA
buffer array
INVA
inverter array
ANDA
AND gate array
NANDA
NAND gate array
ORA
OR gate array
NORA
NOR gate array
XORA
exclusive OR gate array
NXORA
exclusive NOR gate array
AO
AND-OR compound gate
OA
OR-AND compound gate
AOI
AND-NOR compound gate
OAI
OR-NAND compound gate
331
Chapter 7
Digital device modeling
Product Version 10.5
Table 7-1 Digital primitives summary
Type
Description
Tristate gates
BUF3
buffer
INV3
inverter
AND3
AND gate
NAND3
NAND gate
OR3
OR gate
NOR3
NOR gate
XOR3
exclusive OR gate
NXOR3
exclusive NOR gate
BUF3A
buffer array
INV3A
inverter array
AND3A
AND gate array
NAND3A
NAND gate array
OR3A
OR gate array
NOR3A
NOR gate array
XOR3A
exclusive OR gate array
NXOR3A
exclusive NOR gate array
Bidirectional transfer gates
NBTG
N-channel transfer gate
PBTG
P-channel transfer gate
Flip-flops and latches
332
JKFF
J-K, negative-edge triggered
DFF
D-type, positive-edge triggered
SRFF
S-R gated latch
DLTCH
D gated latch
PSpice User's Guide
Product Version 10.5
Chapter overview
Table 7-1 Digital primitives summary
Type
Description
Pullup/pulldown resistors
PULLUP
pullup resistor array
PULLDN
pulldown resistor array
Delay lines
DLYLINE
delay line
Programmable logic arrays
PLAND
AND array
PLOR
OR array
PLXOR
exclusive OR array
PLNAND
NAND array
PLNOR
NOR array
PLNXOR
exclusive NOR array
PLANDC
AND array, true and complement
PLORC
OR array, true and complement
PLXORC
exclusive OR array, true and complement
PLNANDC
NAND array, true and complement
PLNORC
NOR array, true and complement
PLNXORC
exclusive NOR array, true and
complement
Memory
ROM
read-only memory
RAM
random access read-write memory
Multi-Bit A/D & D/A Converters
ADC
multi-bit A/D converter
DAC
multi-bit D/A converter
Behavioral
PSpice User's Guide
333
Chapter 7
Digital device modeling
Product Version 10.5
Table 7-1 Digital primitives summary
Type
Description
LOGICEXP
logic expression
PINDLY
pin-to-pin delay
CONSTRAINT
constraint checking
The format for digital primitives is similar to that for analog
devices. One difference is that most digital primitives require
two models instead of one:
■
The timing model, which specifies propagation delays
and timing constraints such as setup and hold times.
■
The I/O model, which specifies information specific to
the device’s input/output characteristics.
The reason for having two models is that, while timing
information is specific to a device, the input/output
characteristics are specific to a whole logic family. Thus, many
devices in the same family reference the same I/O model, but
each device has its own timing model.
Figure 7-1 presents an overview of a digital device definition
in terms of its primitives and underlying model attributes.
These models are discussed further on Timing model on
page 339 and Input/Output model on page 346.
Digital primitive syntax
The general digital primitive format is shown below. For
specific information on each primitive type see the online
PSpice Reference Guide. Note that some digital primitives,
such as pullups, do not have Timing models. See Timing
model on page 339 for more information.
U<name> <primitive type> [( <parameter value>* )]
+ <digital power node> <digital ground node>
+ <node>*
+ <Timing Model name> <I/O Model name>
+ [MNTYMXDLY=<delay select value>]
+ [IO_LEVEL=<interface subckt select value>]
where
334
PSpice User's Guide
Product Version 10.5
Chapter overview
<primitive type> [( <parameter value>* )]
is the type of digital device, such as NAND, JKFF, or INV. It is
followed by zero or more parameters specific to the primitive
type, such as number of inputs. The number and meaning of
the parameters depends on the primitive type.
<digital power node> <digital ground node>
are the nodes used by the interface subcircuits which
connect analog nodes to digital nodes or vice versa.
<node>*
is one or more input and output nodes. The number of
nodes depends on the primitive type and its parameters.
Analog devices, digital devices, or both may be
connected to a node. If a node has both analog and digital
connections, then PSpice A/D automatically inserts an
interface subcircuit to translate between digital output
states and voltages.
<Timing model name>
is the name of a timing model that describes the device’s
timing characteristics, such as propagation delay and
setup and hold times. Each timing parameter has a
minimum, typical, and maximum value which may be
selected during analysis setup.
This type of Timing model and its parameters are specific
to each primitive type and are discussed in the online
PSpice Reference Guide.
<I/O model name>
is the name of an I/O model that describes the device’s
loading and driving characteristics. I/O models also
contain the names of up to four DtoA and AtoD interface
subcircuits, which are automatically called by PSpice A/D
to handle analog/digital interface nodes. See Input/Output
model on page 346 for more information.
PSpice User's Guide
335
Chapter 7
Digital device modeling
Product Version 10.5
Digital device
.subckt 7400 A B Y
+ params: MNTYMXDLY=0 IO_LEVEL=0
+ optional: DPWR=$G_DPWR DGND=$G_DGND
U1 NAND(2) DPWR DGND A B Y
IO_STD
+ D_7400
+ MNTYMXDLY={MNTYMXDLY} IO_LEVEL={IO_LEVEL}
Timing model
I/O model
.model IO_STD uio (
+ drvh=96.4 drvl=104
+ AtoD1="AtoD_STD"
AtoD2="AtoD_STD_NX"
+ AtoD3="AtoD_STD"
AtoD4="AtoD_STD_NX"
+ DtoA1="DtoA_STD"
DtoA2="DtoA_STD"
+ DtoA3="DtoA_STD"
DtoA4="DtoA_STD"
+ tswhl1=1.373ns
tswlh1=3.382ns
...
+ DIGPOWER="DIGIFPWR" )
.model D_7400 ugate (
+ tplhty=11ns tplhmx=22ns
+ tphlty=7ns tphlmx=15ns )
AtoD interface subcircuit
DtoA interface subcircuit
.subckt AtoD_STD A D DPWR DGND
+ .params: CAPACITANCE=0
O0 A DGND DO74 DGTLNET=D IO_STD
C1 A DGND {CAPACITANCE+0.1pF}
.ends
Digital output (AtoD) model
.model DO74 doutput(
+ s0name="X"
s0vlo=0.8
+ s1name="0"
s1vlo=0.0
+ s2name="R"
s2vlo=0.8
+ s3name="R"
s3vlo=1.3
+ s4name="X"
s4vlo=0.8
+ s5name="1"
s5vlo=2.0
+ s6name="F"
s6vlo=1.3
+ s7name="F"
s7vlo=0.8
+)
.subckt DotA_STD D A DPWR DGND
+ params: DRVL=0 DRVH=0 CAPACITANCE=0
N1 A DGND DPWR DIN74 DGTLNET=D IO_STD
C1 A DGND {CAPACITANCE+0.1pF}
.ends
Digital input (DtoA) model
s0vhi=2.0
s1vhi=0.8
s2vhi=1.4
s3vhi=2.0
s4vhi=2.0
s5vhi=7.0
s6vhi=2.0
s7vhi=1.4
.model DIN74 dinput(
+ s0name="0" s0tsw=3.5ns
+ s1name="1" s1tsw=5.5ns
+ s2name="X" s2tsw=3.5ns
+ s3name="R" s3tsw=3.5ns
+ s4name="F" s4tsw=3.5ns
+ s5name="Z" s5tsw=3.5ns
+)
s0rlo=7.13
s1rlo=467
s2rlo=42.9
s3rlo=42.9
s4rlo=42.9
s5rlo=200K
s0rhi=389
s1rhi=200
s2rhi=116
s3rhi=116
s4rhi=116
s5rhi=200K
Figure 7-1 Elements of a digital device definition
MNTYMXDLY
is an optional device parameter that selects either the
minimum, typical, or maximum delay values from the
336
PSpice User's Guide
Product Version 10.5
Chapter overview
device’s timing model. If not specified, MNTYMXDLY
defaults to 0. Valid values are:
0
=
1
2
3
4
=
=
=
=
the current value of the circuit-wide
DIGMNTYMX option (default=2)
minimum
typical
maximum
worst-case timing (min-max)
IO_LEVEL
is an optional device parameter that selects one of the
four AtoD or DtoA interface subcircuits from the device’s
I/O model. PSpice A/D calls the selected subcircuit
automatically in the event a node connecting to the
primitive also connects to an analog device. If not
specified, IO_LEVEL defaults to 0. Valid values are:
0
=
1
2
3
4
=
=
=
=
the current value of the circuit-wide
DIGIOLVL option (default=1)
AtoD1/DtoA1
AtoD2/DtoA2
AtoD3/DtoA3
AtoD4/DtoA4
Following are some simple examples of “U” device
declarations:
U1 NAND(2) $G_DPWR $G_DGND 1 2 10 D0_GATE IO_DFT
U2 JKFF(1) $G_DPWR $G_DGND 3 5 200 3 3 10 2 D_293ASTD
+ IO_STD
U3 INV $G_DPWR $G_DGND IN OUT D_INV IO_INV MNTYMXDLY=3
+ IO_LEVEL=2
For example, the 74393 part could be defined as a subcircuit
composed of “U” devices as shown below.
.subckt 74393 A CLR QA QB QC QD
+ optional: DPWR=$G_DPWR DGND=$G_DGND
+ params: MNTYMXDLY=0 IO_LEVEL=0
UINV inv DPWR DGND
+ CLR
CLRBAR D0_GATE IO_STD
+ IO_LEVEL={IO_LEVEL}
U1 jkff(1) DPWR DGND
+ $D_HI CLRBAR A
$D_HI $D_HI
+ QA_BUF $D_NC D_393_1 IO_STD
PSpice User's Guide
337
Chapter 7
Digital device modeling
Product Version 10.5
+ MNTYMXDLY={MNTYMXDLY}
+ IO_LEVEL={IO_LEVEL}
U2 jkff(1) DPWR DGND
+ $D_HI CLRBAR QA_BUF
$D_HI $D_HI
+ QB_BUF $D_NC D_393_2 IO_STD
+ MNTYMXDLY={MNTYMXDLY}
U3 jkff(1) DPWR DGND
+ $D_HI CLRBAR QB_BUF
$D_HI $D_HI
+ QC_BUF $D_NC D_393_2 IO_STD
+ MNTYMXDLY={MNTYMXDLY}
U4 jkff(1) DPWR DGND
+ $D_HI CLRBAR QC_BUF
$D_HI $D_HI
+ QD_BUF $D_NC D_393_3 IO_STD
+ MNTYMXDLY={MNTYMXDLY}
UBUFF bufa(4) DPWR DGND
+ QA_BUF QB_BUF QC_BUF QD_BUF
+ QA QB QC QD D_393_4 IO_STD
+ MNTYMXDLY={MNTYMXDLY}
+ IO_LEVEL={IO_LEVEL}
.ends
When adding digital parts to the part libraries, you must create
corresponding digital device models by connecting U devices
in a subcircuit definition similar to the one shown above. You
should save these in your own custom model library, which
you can then configure for use with a given design.
338
PSpice User's Guide
Product Version 10.5
Chapter overview
Timing characteristics
A digital device model’s timing behavior can be defined in one
of two ways:
■
Most primitives have an associated Timing model, in
which propagation delays and timing constraints (such as
setup/hold times) are specified. This method is used
when it is easy to partition delays among individual
primitives; typically when the number of primitives is
small.
■
Use the PINDLY and CONSTRAINT primitives, which can
directly model pin-to-pin delays and timing constraints for
the whole device model. With this method, all other
functional primitives operate in zero delay. Refer to the
online PSpice Reference Guide for a detailed
discussion on these two primitives.
In addition to explicit propagation delays, other factors, such
as output loads, can affect the total propagation delay through
a device.
Timing model
With the exception of the PULLUP, PULLDN, and PINDLY
devices, all digital primitives have a Timing model which
provides timing parameters to the simulator. The Timing
model for each primitive type is unique. That is, the model
name and the parameters that can be defined for that model
vary with the primitive type.
Within a Timing model, there may be one or more types of
parameters:
PSpice User's Guide
■
Propagation delays (TP)
■
Setup times (TSU)
■
Hold times (TH)
■
Pulse widths (TW)
■
Switching times (TSW)
339
Chapter 7
Digital device modeling
Product Version 10.5
Each parameter is further divided into three values: minimum
(MN), typical (TY), and maximum (MX). For example, the
typical low-to-high propagation delay on a gate is specified as
the parameter TPLHTY. The minimum data-to-clock setup
time on a flip-flop is specified as the parameter TSUDCLKMN.
Several timing models are used by digital device 74393 from
the model libraries. One of them, D_393_1, is shown below for
an edge-triggered flip-flop.
.model D_393_1 ueff
+ tppcqhlty=18ns
+ tpclkqlhty=6ns
+ tpclkqhlty=7ns
+ twclkhmn=20ns
+ twpclmn=20ns
+ )
(
tppcqhlmx=33ns
tpclkqlhmx=14ns
tpclkqhlmx=14ns
twclklmn=20ns
tsudclkmn=25ns
When creating your own digital device models, you can create
Timing models like these for the primitives you are using.
PSpice recommends that you save these in your own custom
model library, which you can then configure for use with a
given design.
One or more parameters may be missing from the Timing
model definition. Data books do not always provide all three
(minimum, typical, and maximum) timing specifications. The
way the simulator handles missing parameters depends on
the type of parameter.
For a description of Timing model parameters, see the specific
primitive type under U devices in the online PSpice
Reference Guide.
Treatment of unspecified propagation delays
Often, only the typical and maximum delays are specified in
data books. If, in this case, the simulator were to assume that
the unspecified minimum delay defaults to zero, the logic in
certain circuits could break down.
For this reason, the simulator provides two configurable
options, DIGMNTYSCALE and DIGTYMXSCALE, which are
used to extrapolate unspecified propagation delays in the
Timing models.
340
PSpice User's Guide
Product Version 10.5
Chapter overview
Note: This discussion applies only to propagation delay
parameters (TP). All other timing parameters, such as
setup/hold times and pulse widths are handled
differently, and are discussed in the following section.
DIGMNTYSCALE
This option computes the minimum delay when a typical delay
is known, using the formula:
TPxxMN = DIGMNTYSCALE ⋅ TPxxTY
DIGMNTYSCALE defaults to the value 0.4, or 40% of the
typical delay. Its value must be between 0.0 and 1.0.
DIGTYMXSCALE
This option computes the maximum delay from a typical delay,
using the formula
TPxxMX = DIGTYMXSCALE ⋅ TPxxTY
DIGTYMXSCALE defaults to the value 1.6. Its value must be
greater than 1.0.
When a typical delay is unspecified, its value is derived from
the minimum and/or maximum delays, in one of the following
ways. If both the minimum and maximum delays are known,
the typical delay is the average of these two values. If only the
minimum delay is known, the typical delay is derived using the
value of the DIGMNTYSCALE option. Likewise, if only the
maximum delay is specified, the typical delay is derived using
DIGTYMXSCALE. Obviously, if no values are specified, all
three delays will default to zero.
Treatment of unspecified timing constraints
The remaining timing constraint parameters are handled
differently than the propagation delays. Often, data books
state pulse widths, setup times, and hold times as a minimum
value. These parameters do not lend themselves to the
extrapolation method used for propagation delays.
PSpice User's Guide
341
Chapter 7
Digital device modeling
Product Version 10.5
Instead, when one or more timing constraints are omitted, the
simulator uses the following steps to fill in the missing values:
■
If the minimum value is omitted, it defaults to zero.
■
If the maximum value is omitted, it takes on the typical
value if one was specified, otherwise it takes on the
minimum value.
■
If the typical value is omitted, it is computed as the
average of the minimum and maximum values.
Propagation delay calculation
The timing characteristics of digital primitives are determined
by both the timing models and the I/O models. Timing models
specify propagation delays and timing constraints such as
setup and hold times. I/O models specify input and output
loading, driving resistances, and switching times.
When a device’s output connects to another digital device, the
total propagation delay through a device is determined by
adding the loading delay (on the output terminal) to the delay
specified in the device’s timing model. Loading delay is
calculated from the total load on the output and the device’s
driving resistances. The total load on an output is found by
summing the output and input loads (OUTLD and INLD in the
I/O model) of all devices connected to that output. This total
load, combined with the device’s driving resistances (DRVL
and DRVH in the I/O model), allows the loading delay to be
calculated:
Loading delay = RDRIVE·CTOTAL·ln(2)
The loading delay is calculated for each output terminal of
every device before the simulation begins. The total
propagation delay is easily calculated during the simulation by
adding the pre-calculated loading delay to the device’s timing
delay. However, for any individual timing delay specification
(e.g., TPLH) having a value of 0, the loading delay is not
used.
When outputs connect to analog devices, the propagation
delay is reduced by the switching times specified in the I/O
342
PSpice User's Guide
Product Version 10.5
Chapter overview
model. See Input/Output characteristics on page 346 for more
information.
Inertial and transport delay
The simulator uses two different types of internal delay
functions when simulating the digital portion of the circuit:
inertial delay and transport delay. The application of these
concepts is embodied within the implementation of the digital
primitives within the simulator. Therefore, they are not
user-selectable.
Inertial delay
The simulation of a device may be described as the
application of some stimulus (S) to a function (F) and
predicting the response (R).
S
F
If this device is electrical in nature, application of the stimulus
implies that energy will be imparted to the device to cause it to
change state. The amount of such energy is a function of the
signal’s amplitude and duration. If the stimulus is applied to
the device for a length of time that is too short, the device will
not switch. The minimum duration required for an input
change to have an effect on a device’s output state is called
the inertial delay of the device. For digital simulation, all
delay parameters specified in timing models are considered
inertial, with the exception of the delay line primitive, DLYLINE.
To model the noise immunity behavior of digital devices
correctly, the TPWRT (pulse width rejection threshold)
parameter can be set in the digital device’s I/O model. When
pulse width ≥ TPWRT and pulse width < propagation
delay, then the device generates either a 0-R-0, 1-F-1, or an
X pulse.
PSpice User's Guide
343
Chapter 7
Digital device modeling
Product Version 10.5
This example shows normal operation in which a pulse of 20
nsec width is applied to a BUF primitive having propagation
delays of 10 nsec. TPWRT is not set.
20
40
30
50
TPLHTY=10
TPHLTY=10
(TPWRT not set)
The same device with a short pulse applied produces no
output change.
20
22
TPLHTY=10
TPHLTY=10
(TPWRT not set)
However, if TPWRT is assigned a numerical value (1 or 2 for
this example), then the device outputs a glitch.
20
22
30
32
TPLHTY=10
TPHLTY=10
TPWRT=1
Transport delay
The delay line primitive is the only simulator model that can
propagate any width pulse applied to its input. Its function is to
skew the applied stimulus by some constant time value. For
example:
T
0
344
2
6
8
12
14
DLYTY=4
4
6
10 12
16 18
PSpice User's Guide
Product Version 10.5
Chapter overview
See the DLYLINE digital primitive in the online PSpice
Reference Guide.
PSpice User's Guide
345
Chapter 7
Digital device modeling
Product Version 10.5
Input/Output characteristics
A digital device model’s input/output characteristics are
defined by the I/O model that it references. Some
characteristics, such as output drive resistance and loading
capacitances, apply to digital simulation. Others, such as the
interface subcircuits and the power supplies, apply only to
mixed analog/digital simulation.
This section describes in detail:
■
the I/O model
■
the relationship between drive resistances and output
strengths
■
charge storage on digital nets
■
the format of the interface subcircuits
Input/Output model
I/O models are common to entire logic families. For example,
in the model libraries, there are only four I/O models for the
entire 74LS family: IO_LS, for standard inputs and outputs;
IO_LS_OC, for standard inputs and open-collector outputs;
IO_LS_ST, for Schmitt trigger inputs and standard outputs;
and IO_LS_OC_ST, for Schmitt trigger inputs and
open-collector outputs. In contrast, timing models are unique
to each device.
I/O models are specified as
.MODEL <I/O model name> UIO [model parameters]*
where valid model parameters are described in Table 7-2.
INLD and OUTLD
These are used in the calculation of loading capacitance,
which factors into the propagation delay discussed under
timing models on Timing model on page 339. Note that INLD
346
PSpice User's Guide
Product Version 10.5
Chapter overview
does not apply to stimulus generators because they have no
input nodes.
DRVH and DRVL
These are used to determine the strength of the output.
Strengths are discussed on Defining Output Strengths on
page 350.
DRVZ, INR, and TSTOREMN
These are used to determine which nets should be simulated
as charge storage nets. These are discussed in Charge
storage nets on page 352.
TPWRT
This is used to specify the pulse width above which the noise
immunity behavior of a device is to be considered. See Inertial
delay on page 343 on inertial delay for detail.
The following UIO model parameters are needed only when
creating models for use in mixed-signal simulations, and
therefore only apply to PSpice A/D simulations.
AtoD1 through AtoD4, and DtoA1 through DtoA4
These are used to hold the names of interface subcircuits.
Note that AtoD1 through AtoD4 do not apply to stimulus
generators because digital stimuli have no input nodes.
DIGPOWER
This is used to specify the name of the digital power supply
PSpice A/D should call if one of the AtoD or DtoA interface
subcircuits is called.
PSpice User's Guide
347
Chapter 7
Digital device modeling
Product Version 10.5
TSWLHn and TSWHLn
These switching times are subtracted from a device’s
propagation delay on the outputs which connect to interface
nodes. This compensates for the time it takes the DtoA device
to change its output voltage from its current level to that of the
switching threshold. By subtracting the switching time from the
propagation delay, the analog signal reaches the switching
threshold at the correct time (that is, at the exact time of the
digital transition). The values for these model parameters
should be obtained by measuring the time it takes the analog
output of the DtoA (with a nominal analog load attached) to
change to the switching threshold after its digital input
changes. If the switching time is larger than the propagation
delay for an output, no warning is issued, and a delay of zero
is used.
When creating your own digital device models, you can create
I/O models like these for the primitives you are using. We
recommend that you save these in your own custom model
library, which you can then configure for use with a given
design.
See the online PSpice Reference Guide for more
information on units and defaults for these parameters.
Note: The switching time parameters are not used when the
output drives a digital node.
Table 7-2 Digital I/O model parameters
348
UIO model
parameter
Description
INLD
input load capacitance
OUTLD
output load capacitance
DRVH
output high level resistance
DRVL
output low level resistance
DRVZ
output Z-state leakage resistance
INR
input leakage resistance
PSpice User's Guide
Product Version 10.5
Chapter overview
Table 7-2 Digital I/O model parameters, continued
UIO model
parameter
Description
TSTOREMN
minimum storage time for net to be
simulated as a charge
TPWRT
pulse width rejection threshold
AtoD1 (Level 1)
name of AtoD interface subcircuit
DtoA1 (Level 1)
name of DtoA interface subcircuit
AtoD2 (Level 2)
name of AtoD interface subcircuit
DtoA2 (Level 2)
name of DtoA interface subcircuit
AtoD3 (Level 3)
name of AtoD interface subcircuit
DtoA3 (Level 3)
name of DtoA interface subcircuit
AtoD4 (Level 4)
name of AtoD interface subcircuit
DtoA4 (Level 4)
name of DtoA interface subcircuit
DIGPOWER
name of power supply subcircuit
TSWLH1
switching time low to high for DtoA1
TSWLH2
switching time low to high for DtoA2
TSWLH3
switching time low to high for DtoA3
TSWLH4
switching time low to high for DtoA4
TSWHL1
switching time high to low for DtoA1
TSWHL2
switching time high to low for DtoA2
TSWHL3
switching time high to low for DtoA3
TSWHL4
switching time high to low for DtoA4
The digital primitives comprising the 74393 part reference the
IO_STD I/O model in the model libraries as shown:
.model IO_STD uio (
+ drvh=96.4
drvl=104
+ AtoD1="AtoD_STD" AtoD2="AtoD_STD_NX"
+ AtoD3="AtoD_STD" AtoD4="AtoD_STD_NX"
+ DtoA1="DtoA_STD" DtoA2="DtoA_STD"
+ DtoA3="DtoA_STD" DtoA4="DtoA_STD"
+ tswhl1=1.373ns
tswlh1=3.382ns
PSpice User's Guide
349
Chapter 7
Digital device modeling
Product Version 10.5
+
+
+
+
tswhl2=1.346ns
tswhl3=1.511ns
tswhl4=1.487ns
)
tswlh2=3.424ns
tswlh3=3.517ns
tswlh4=3.564ns
Defining Output Strengths
The goal of running simulations is to calculate values for each
node in the circuit. For analog nodes, the values are voltages.
For digital nodes, these values are states. The state of a
digital node is calculated from the output strengths of the
devices driving the node and the logic level of the node. Node
strength calculations are described in Chapter 14, “Digital
simulation.”
The purpose of strengths is to allow the simulator to find the
value of a node when more than one output is driving it. A
common example is a bus line which is driven by more than
one tristate driver. Under normal circumstances, all drivers
except one are driving at the Z (high impedance) strength.
Thus, the bus line will take on the value of the one gate that is
driving at a higher strength (lower impedance).
Another example is a bus line connected to several open
collector output devices and a digital pullup resistor. The
pullup resistor outputs a 1 level at a weak (but non-Z) strength.
If all of the open-collector devices are outputting at Z strength,
then the node will have a 1 level because of the pullup resistor.
If any of the open collectors output a 0, at a higher strength
than the pullup resistor, then the 0 will overpower the weak 1
from the pullup, and the node will be a 0 level.
Configuring the strength scale
The 64 strengths are determined by two configurable options:
DIGDRVZ and DIGDRVF. You can set these options in the
Simulation Settings dialog box in PSpice A/D.
DIGDRVZ defines the impedance of the Z strength, and
DIGDRVF defines the impedance of the forcing strength.
These two values define a logarithmic scale consisting of 64
ranges of impedance values. By default, DIGDRVZ is 20
kohms and DIGDRVF is 2 ohms. The larger the range
350
PSpice User's Guide
Product Version 10.5
Chapter overview
between DIGDRVZ and DIGDRVF, the larger the range of
impedance values in each of the 64 strengths.
Determining the strength of a device output
The simulator uses the value of the DRVH (high-level driving
resistance) or DRVL (low-level driving resistance) parameters
from the device’s I/O model. If the level of the output is a 1, the
simulator obtains the strength by finding the bin which
contains the value of the DRVH parameter. Likewise, if the
level is a 0, the simulator uses the value of the DRVL
parameter to obtain the strength.
See Input/Output model on page 346 for more information.
Output
Drive
Output
Strength
Output
Drive
Output
Strength
DIGDRVF
63
DIGDRVF
63
.
.
.
.
.
.
Higher
Strength
(DRVH)
Level 1
Strength
Level 0
Higher
Strength Impedance
.
.
.
.
.
.
DIGDRVZ
(DRVL)
0
DIGDRVZ
0
Figure 7-2 Level 1 and 0 strength determination.
Note that if the values of DRVH and DRVL in the I/O model are
different, it is possible for the 1 and 0 levels to have different
strengths. This is useful for open-collector devices, where the
0 level is at a higher strength than the 1 level (which drives at
the Z strength).
Drive impedances which are higher than the value of
DIGDRVZ are assigned the Z strength (0). Likewise, drive
impedances lower than the value of DIGDRVF are assigned
the forcing strength (63).
PSpice User's Guide
351
Chapter 7
Digital device modeling
Product Version 10.5
Controlling overdrive
During a simulation, the simulator uses only the strength
range number (0-63) to compare the driving strength of
outputs. The simulator allows you to control how much
stronger an output must be before it overdrives the other
outputs driving the same node. This is controlled with the
configurable DIGOVRDRV option. By default, DIGOVRDRV is
3, meaning that the strength value assigned to an output must
be at least 3 greater than all other drivers before it determines
the level of the node.
The accuracy of the DIGOVRDRV strength comparison is
limited by the size of the strength range, DIGDRVZ through
DIGDRVF. The default drive range of 2 ohms to 20,000 ohms
gives strength ranges of 7.5%. The accuracy of the strength
comparison is 15%. In other words, depending on the
particular values of DRVH and DRVL, it might take as much as
a factor of 3.45 to overdrive a signal, or as little as a factor of
2.55. The accuracy of the comparison increases as the ratio
between DIGDRVF and DIGDRVZ decreases.
You can set the DRVH, DRVL, DIGDRVF, DIGDRVZ, and
DIGOVRDRV options in the Simulation Settings dialog box in
PSpice A/D.
Charge storage nets
The ability to model charge storage on digital nets is useful for
engineers who are designing dynamic MOS integrated
circuits. In such circuits, it is common for the designer to
temporarily store a one or zero on a net by driving the net to
the appropriate voltage and then turning off the drive. The
charge which is trapped on the net causes the net’s voltage to
remain unchanged for some time after the net is no longer
driven. The technique is not normally used on PCB nets
because sub-nanoampere input and output leakage currents
would be required, as well as low coupling from adjacent
signals.
The simulator models the stored charge nets using a
simplified switch-level simulation technique. A normalized
(with respect to power supply) charge or discharge current is
352
PSpice User's Guide
Product Version 10.5
Chapter overview
calculated for each output or transfer gate attached to the net.
This current, divided by the net’s total capacitance, is
integrated and recalculated at intervals which are appropriate
for the particular net. The net’s digital level is determined by
the normalized voltage on the net. Only the digital level (1, 0,
R, F, X) on the net is used by device inputs attached to the net.
This technique allows accurate simulation of networks of
transfer gates and capacitive loads. The sharing of charge
among several nets which are connected by transfer gates is
handled properly because the simulation method calculates
the charge transferred between the nets, and maintains a
floating-point value for the charge on the net (not just a one or
zero). Because of the increased computation, it takes the
simulator longer to simulate charge storage nets than normal
digital nets. However, charge storage nets are simulated much
faster than analog nets.
The I/O model parameters INR, DRVZ, and TSTOREMN (see
Table 7-2 on page 348) are used by the simulator to determine
which nets should be simulated as charge storage nets. The
simulator will simulate charge storage only for a net which has
some devices attached to it which can be high impedance (Z),
and which has a storage time greater than or equal to the
smallest TSTOREMN of all inputs attached to the net. The
storage time is calculated as the total capacitance (sum of all
INLD and OUTLD values for attached inputs and outputs)
multiplied by the total leakage resistance for the net (the
parallel combination of all INR and DRVZ values for attached
inputs and outputs).
Note: The default values provided by the UIO model will not
allow the use of charge-storage simulation
techniques—even with circuits using non-PSpice
libraries of digital devices. This is appropriate, since
these libraries are usually for PCB-based designs.
Creating your own interface subcircuits for
additional technologies
If you are creating custom digital parts for a technology which
is not in the model libraries, you may also need to create AtoD
and DtoA subcircuits. The new subcircuits need to be
PSpice User's Guide
353
Chapter 7
Digital device modeling
Product Version 10.5
referenced by the I/O models for that technology. The AtoD
and DtoA interfaces have specific formats, such as node order
and parameters, which are expected by PSpice A/D for
mixed-signal simulations.
If you are creating parts in one of the logic families already in
the model libraries, you should reference the existing I/O
models appropriate to that family. The I/O models, in turn,
automatically reference the correct interface subcircuits for
that family. These, too, are already contained in the model
libraries.
The AtoD interface subcircuit format is shown here:
.SUBCKT ATOD <name suffix>
+ <analog input node>
+ <digital output node>
+ <digital power supply node>
+ <digital ground node>
+ PARAMS: CAPACITANCE=<input load value>
+ {O device, loading capacitor, and other
+ declarations}
.ENDS
It has four nodes as described. The AtoD subcircuit has one
parameter, CAPACITANCE, which corresponds to the input
load. PSpice A/D passes the value of the I/O model parameter
INLD to this parameter when the interface subcircuit is called.
The DtoA interface subcircuit format is shown here:
.SUBCKT DTOA <name suffix>
+ <digital input node> <analog output node>
+ <digital power supply node> <digital
+ ground node>
+ PARAMS: DRVL=<0 level driving resistance>
+ DRVH=<1 level driving resistance>
+ CAPACITANCE=<output load value>
+ {N device, loading capacitor, and other
+ declarations}
.ENDS
It also has four nodes. Unlike the AtoD subcircuit, the DtoA
subcircuit has three parameters. PSpice A/D will pass the
values of the I/O model parameters DRVL, DRVH, and
OUTLD to the interface subcircuit’s DRVL, DRVH, and
CAPACITANCE parameters when it is called.
The library file DIG_IO.LIB contains the I/O models and
interface subcircuits for all logic families supported in the
model libraries. You should refer to this file for examples of the
354
PSpice User's Guide
Product Version 10.5
Chapter overview
I/O models, interface subcircuits, and the proper use of N and
O devices.
Shown below are the I/O model and AtoD interface subcircuit
definition used by the primitives describing the 74393 part.
.model IO_STD uio (
+ drvh=96.4
drvl=104
+ AtoD1="AtoD_STD"
AtoD2="AtoD_STD_NX"
+ AtoD3="AtoD_STD"
AtoD4="AtoD_STD_NX"
+ DtoA1="DtoA_STD"
DtoA2="DtoA_STD"
+ DtoA3="DtoA_STD"
DtoA4="DtoA_STD"
+ tswhl1=1.373
tswlh1=3.382ns
+ tswhl2=1.346ns
tswlh2=3.424ns
+ tswhl3=1.511ns
tswlh3=3.517ns
+ tswhl4=1.487ns
tswlh4=3.564ns
+ )
.subckt AtoD_STD A D DPWR DGND
+ params: CAPACITANCE=0
*
O0 A DGND DO74 DGTLNET=D IO_STD
C1 A 0 {CAPACITANCE+0.1pF}
.ends
If an instance of the 74393 part is connected to an analog part
via node AD_NODE, PSpice A/D generates an interface block
using the I/O model specified by the digital primitive actually at
the interface. Suppose that U1 is the primitive connected at
AD_NODE (see the 74393 subcircuit definition on page 337),
and that the IO_LEVEL is set to 1. PSpice A/D determines that
IO_STD is the I/O model used by U1. Notice how IO_STD
identifies the interface subcircuit names AtoD_STD and
DtoA_STD to be used for level 1 subcircuit selection. If the
connection with U1 is an input (such as a clock line), PSpice
A/D creates an instance of the subcircuit AtoD_STD:
X$AD_NODE_AtoD1 AD_NODE AD_NODE$AtoD $G_DPWR
+ $G_DGND
+ AtoD_STD
+ PARAMS: CAPACITANCE=0
The AtoD_STD interface subcircuit references the DO74
model in its PSpice A/D O device declaration. This model,
stated elsewhere in the model libraries, describes how to
translate an analog signal on the analog side of an interface
node, to a digital state on the digital side of an interface node.
.model DO74 doutput
+ s0name="X" s0vlo=0.8
+ s1name="0" s1vlo=-1.5
+ s2name="R" s2vlo=0.8
+ s3name="R" s3vlo=1.3
+ s4name="X" s4vlo=0.8
PSpice User's Guide
s0vhi=2.0
s1vhi=0.8
s2vhi=1.4
s3vhi=2.0
s4vhi=2.0
355
Chapter 7
Digital device modeling
Product Version 10.5
+
+
+
+
s5name="1"
s6name="F"
s7name="F"
s5vlo=2.0
s6vlo=1.3
s7vlo=0.8
s5vhi=7.0
s6vhi=2.0
s7vhi=1.4
The DOUTPUT model parameters are described under O
devices in the online PSpice Reference Guide.
Supposing the output of the 74393 is connected to an analog
part via the digital primitive UBUFF. At IO_LEVEL set to 1,
PSpice A/D determines that the DtoA_STD interface
subcircuit identified in the IO_STD model, should be used.
.subckt DtoA_STD D A DPWR DGND
+ params: DRVL=0 DRVH=0 CAPACITANCE=0
*
N1 A DGND DPWR DIN74 DGTLNET=D IO_STD
C1 A DGND {CAPACITANCE+0.1pF}
.ends
For this subcircuit, the DRVH and DRVL parameters values
specified in the IO_STD model would be passed to it. (The
interface subcircuits in the model libraries do not currently use
these values.)
The DtoA_STD interface subcircuit references the DIN74
model in its PSpice A/D N device declaration. This model,
stated elsewhere in the libraries, describes how to translate a
digital state into a voltage and impedance.
.model DIN74 dinput (
+ s0name="0" s0tsw=3.5ns s0rlo=7.13
+ s0rhi=389 ; 7ohm, 0.09v
+ s1name="1" s1tsw=5.5ns s1rlo=467
+ s1rhi=200 ; 140ohm, 3.5v
+ s2name="X" s2tsw=3.5ns s2rlo=42.9
+ s2rhi=116 ; 31.3ohm, 1.35v
+ s3name="R" s3tsw=3.5ns s3rlo=42.9
+ s3rhi=116 ; 31.3ohm, 1.35v
+ s4name="F" s4tsw=3.5ns s4rlo=42.9
+ s4rhi=116 ; 31.3ohm, 1.35v
+ s5name="Z" s5tsw=3.5ns s5rlo=200K
+ s5rhi=200K
+)
The DINPUT model parameters are described under PSpice
A/D N devices in the online PSpice Reference Guide.
Each state is turned into a pullup and pulldown resistor pair to
provide the correct voltage and impedance. The Z state is
accounted for as well as the 0, 1, and X logic levels.
356
PSpice User's Guide
Product Version 10.5
Chapter overview
You can create your own interface subcircuits, DINPUT
models, DOUTPUT models, and I/O models like these for
technologies not currently supported in the model libraries.
We recommend that you save these in your own custom
model library, which you can then configure for use with a
given design.
PSpice User's Guide
357
Chapter 7
Digital device modeling
Product Version 10.5
Creating a digital model using the PINDLY and LOGICEXP
primitives
Unlike the majority of analog device types, the bulk of digital
devices are not primitives that are compiled into the simulator.
Instead, most digital models are macro models or subcircuits
that are built from a few primitive devices.
These subcircuits reference interface and timing models to
handle the D-to-A and A-to-D interfaces and the overall timing
parameters of the physical device. For most families of digital
components, the interface models are already defined and
available in the DIG_IO.LIB library, which is supplied with all
digital and mixed-signal packages. If you are unsure of the
exact name of the interface model you need to use, use a text
editor to look in DIG_IO.LIB.
For instance, if you are trying to model a 74LS component that
is not already in a library, open DIG_IO.LIB with your text
editor and search for 74LS to get the interface models for the
74LS family. You can also read the information at the
beginning of the file which explains many of the terms and
uses for the I/O models.
In the past, the timing model has presented the greatest
challenge when trying to model a digital component. This was
due to the delays of a component being distributed among the
various gates. Recently, the ability to model digital
components using logic expressions (LOGICEXP) and
pin-to-pin delays (PINDLY) has been added to the simulator.
Using the LOGICEXP and PINDLY digital primitives, you can
describe the logic of the device with zero delay and then enter
the timing parameters for the pin-to-pin delays directly from
the manufacturer’s data sheet. Digital primitives still must
reference a standard timing model, but when the PINDLY
device is used, the timing models are simply zero-delay
models that are supplied in DIG_IO.LIB. The default timing
models can be found in the same manner as the standard I/O
models. The PINDLY primitive also incorporates constraint
checking which allows you to enter device data such as pulse
width and setup/hold timing from the data sheet. Then the
simulator can verify that these conditions are met during the
simulation.
358
PSpice User's Guide
Product Version 10.5
Chapter overview
Digital primitives
Primitives in the simulator are devices or functions which are
compiled directly into the code. The primitives serve as
fundamental building blocks for more complex macro models.
There are two types of primitives in the simulator: gate level
and behavioral. A gate level primitive normally refers to an
actual physical device (such as buffers, AND gates, inverters).
A behavioral primitive is not an actual physical device, but
rather helps to define parameters of a higher level model. Just
like gate level primitives, behavioral primitives are intrinsic
functions in the simulator and are treated in much the same
manner. They are included in the gate count for circuit size
and cannot be described by any lower level model.
In our 74160 example (see The TTL Data Book from Texas
Instruments for schematic and description), the four J-K
flip-flops are the four digital gate level primitives. While
flip-flops are physically more complex than gates in terms of
modeling, they are defined on the same level as a gate (for
example, flip-flops are a basic device in the simulator). Since
all four share a common Reset, Clear, and Clock signal, they
can be combined into one statement as an array of flip-flops.
They could just as easily have been written separately, but the
array method is more compact. See the Digital Devices
chapter in the online PSpice Reference Guide for more
information.
Logic expression (LOGICEXP primitive)
Looking at the listing in 74160 example on page 366 and at
the schematic representation of the 74160 subcircuit, you can
see that there are three main parts to the subcircuit. Following
the usual header information, .SUBCKT keyword, subcircuit
name, interface pin list, and parameter list is the LOGICEXP
primitive. It contains everything in the component that can be
expressed in terms of simple combinational logic. The logic
expression device also serves to buffer other input signals that
will go to the PINDLY primitive. In this case, LOGICEXP
buffers the ENP_I, ENT_I, CLK_I, CLRBAR_I, LOADBAR_I,
and four data signals. See the Digital Devices chapter in the
online PSpice Reference Guide for more information.
PSpice User's Guide
359
Chapter 7
Digital device modeling
Product Version 10.5
For our 74160 example, the logic expression (LOGICEXP)
has fourteen inputs and twenty outputs. The inputs are the
nine interface input pins in the subcircuit plus five feedback
signals that come from the flip-flops (QA, QB, QC, QD, and
QDBAR). The flip-flops are primitive devices themselves and
are not part of the logic expression. The outputs are the eight
J-K data inputs to the flip-flops, RCO, the four data lines used
internal to the logic expression (A, B, C, D), and the seven
control lines: CLK, CLKBAR, EN, ENT, ENP, CLRBAR, and
LOADBAR.
The schematic representation of the device shows buffers on
every input signal of the model, while the logic diagram of the
device in the data book shows buffers or inverters on only the
CLRBAR_I, CLK_I, and LOADBAR_I signals. We have added
buffers to the inputs to minimize the insertion of A-to-D
interfaces when the device is driven by analog circuitry. The
best example is the CLK signal. With the buffer in place, if the
CLK signal is analog, one A-to-D interface device will be
inserted into the circuit by the simulator. If the buffer was not
present, then an interface device would be inserted at the CLK
pin of each of the flip-flops. The buffers have no delay
associated with them, but by minimizing the number of A-to-D
interfaces, we speed up the mixed-signal simulation by
reducing the number of necessary calculations. For situations
where the device is only connected to other digital nodes, the
buffers have no effect on the simulation.
The D0_GATE, shown in the listing, is a zero-delay primitive
gate timing model. For most TTL modeling applications, this
only serves as a place holder and is not an active part of the
model. Its function has been replaced by the PINDLY primitive.
The D0_GATE model can be found in the library file
DIG_IO.LIB. For a more detailed description of digital
primitives, see the Digital Devices chapter in the online
PSpice Reference Guide.
IO_STD, shown in the listing, is the standard I/O model. This
determines the A-to-D and D-to-A interface characteristics for
the subcircuit. The device contains family-specific information,
but the models have been created for nearly all of the stock
families. The various I/O models can be found in the library file
DIG_IO.LIB.
360
PSpice User's Guide
Product Version 10.5
Chapter overview
The logic expressions themselves are straightforward. The
first nine are buffering the input signals from outside the
subcircuit. The rest describe the logic of the actual device up
to the flip-flops. By tracing the various paths in the design, you
can derive each of the logic equations.
The D0_EFF timing model, shown in the listing, is a zero-delay
default model already defined in DIG_IO.LIB for use with
flip-flops. All of the delays for the device are defined in the
PINDLY section. The I/O model is IO_STD as identified
previously. We have not specified a MNTYMXDLY or
IO_LEVEL parameter, so the default values are used. For a
more detailed description of the general digital primitives
MNTYMXDLY and IO_LEVEL, see the Digital Devices
chapter in the online PSpice Reference Guide.
The primitive MNTYMXDLY specifies whether to use the
minimum, typical, maximum, or digital worst-case timing
values from the device’s timing model (in this case the PINDLY
device). For the 74160, MNTYMXDLY is set to 0. This means
that it takes on the current value of the DIGMNTYMX
parameter. DIGMNTYMX defaults to 2 (typical timing) unless
specifically changed using the .OPTIONS command.
The primitive IO_LEVEL selects one of four possible A-to-D
and D-to-A interface subcircuits from the device’s I/O model.
In the header of this subcircuit, IO_LEVEL is set to 0. This
means that it takes on the value of the DIGIOLVL parameter.
DIGIOLVL defaults to 1 unless specifically changed using the
.OPTIONS command.
Pin-to-pin delay (PINDLY primitive)
The delay and constraint specifications for the model are
specified using the PINDLY primitive. The PINDLY primitive is
evaluated every time any of its inputs or outputs change. See
the Digital Devices chapter in the online PSpice Reference
Guide for more information.
For the 74160, we have five delay paths, the four flip-flop
outputs to subcircuit outputs QA...QD to QA_O...QD_O, and
RCO to RCO_O. The five paths are seen in the Delay &
Constraint section of the design. For delay paths, the number
PSpice User's Guide
361
Chapter 7
Digital device modeling
Product Version 10.5
of inputs must equal the number of outputs. Since the 74160
does not have TRI-STATE outputs, there are no enable signals
for this example, but there are ten reference nodes. The first
four (CLK, LOADBAR, ENT, and CLRBAR) are used for both
the pin-to-pin delay specification and the constraint checking.
The last six (ENP, A, B, C, D, and EN) are used only for the
constraint checking.
The PINDLY primitive also allows constraint checking of the
model. It can verify the setup, hold times, pulse width, and
frequency. It also has a general mechanism to allow for
user-defined conditions to be reported. The constraint
checking only reports timing violations; it does not affect the
propagation delay or the logic state of the device. Since the
timing parameters are generally specified at the pin level of
the actual device, the checking is normally done at the
interface pins of the subcircuit after the appropriate buffering
has been done.
BOOLEAN
The keyword BOOLEAN begins the boolean assignments
which define temporary variables that can be used later in the
PINDLY primitive. The form is:
boolean variable = {boolean expression}
The curly braces are required.
In the 74160 model, the boolean expressions are actually
reference functions. There are three reference functions
available: CHANGED, CHANGED_LH, and CHANGED_HL.
The format is:
function name (node, delta time)
For our example, we define the variable CLOCK as a logical
TRUE if there has been a LO-to-HI transition of the CLK signal
at simulation time. We define CNTENT as TRUE if there has
been any transition of the ENT signal at the simulation time.
Boolean operators take the following boolean values as
operands:
362
PSpice User's Guide
Product Version 10.5
Chapter overview
■
reference functions
■
transition functions
■
previously assigned boolean variables
■
boolean constants TRUE and FALSE
Transition functions have the general form of:
TRN_pn
For a complete list of reference functions and transition
functions, see the Digital Devices chapter in the online
PSpice Reference Guide.
PINDLY
PINDLY contains the actual delay and constraint expressions
for each of the outputs.
The CASE function defines a more complex, rule-based
<delay expression> and works as a rule section mechanism
for establishing path delays. Each boolean expression in the
CASE function is evaluated in order until one is encountered
that produces a TRUE result. Once a TRUE expression is
found, the delay expression portion of the rule is associated
with the output node being evaluated, and the remainder of
the CASE function is ignored. If none of the expressions
evaluate to TRUE, then the DEFAULT delay is used. Since it is
possible for none of the expressions to yield a TRUE result,
you must include a default delay in every CASE function. Also
note that the expressions must be separated by a comma.
In the PINDLY section of the PINDLY primitive in the model
listing, the four output nodes (QA_O through QD_O) all use
the same delay rules. The CASE function is evaluated
independently for each of the outputs in turn. The first delay
expression is:
CLOCK & LOADBAR=='1 & TRN_LH, DELAY(-1,13NS,20NS)
This means that if CLOCK is TRUE, and LOADBAR is equal
to 1, and QA_O is transitioning from 0 to 1, then the values of
-1, 13ns, and 20ns are used for the MINIMUM, TYPICAL, and
MAXIMUM propagation delay for the CLK-to-QA data output
PSpice User's Guide
363
Chapter 7
Digital device modeling
Product Version 10.5
of the chip. In this case, the manufacturer did not supply a
minimum prop delay, so we used the value -1 to tell the
simulator to derive a value from what was given. If this
statement is TRUE, then the simulator assigns the values and
move on to the CASE function for QB_O and eventually
RCO_O.
For instances where one or more propagation delay
parameters are not supplied by the data sheet, the simulator
derives a value from what is known and the values specified
for the .OPTION DIGMNTYSCALE and DIGTYMXSCALE.
When the typical value for a delay parameter is known but the
minimum is not, the simulator uses the formula:
TPxxMN = DIGMNTYSCALE X TPxxTY
where the value of DIGMNTYSCALE is between 0.1 and 1.0
with the default value being 0.4. If the typical is known and the
maximum is not, then the simulator uses the formula:
TPxxMX = DIGTYMXSCALE X TPxxTY
where the value of DIGTYMXSCALE is greater than 1.0 with
the default being 1.6. If the typical value is not known, and
both the minimum and maximum are, then the typical value
used by the simulator will be the average of the minimum and
maximum propagation delays. If only one of min or max is
known, then the typical delay is calculated using the
appropriate formula as listed above. If all three are unknown,
then they all default to a value of 0.
Constraint checker (CONSTRAINT primitive)
The CONSTRAINT primitive provides a general constraint
checking mechanism to the digital device modeler. It performs
setup and hold time checks, pulse width checks, frequency
checks, and includes a general mechanism to allow
user-defined conditions to be reported. See the Digital
Devices chapter in the online PSpice Reference Guide for
more information.
364
PSpice User's Guide
Product Version 10.5
Chapter overview
Setup_Hold
The expressions in the SETUP_HOLD specification may be
listed in any order.
CLOCK defines the node that is to be used as the reference
for the setup/hold/release specification. The assertion edge
must be LH or HL (for example, a transition from logic state 0
to 1 or from 1 to 0.)
DATA specifies which node(s) is to have its setup/hold time
measured.
SETUPTIME defines the minimum time that all DATA nodes
must be stable prior to the assertion edge of the clock. The
time value must be a nonnegative constant or expression and
is measured in seconds. If the device has different setup/hold
times depending on whether the data is HI or LOW at the clock
change, you can use either or both of the following forms:
SETUPTIME_LO = <time value>
SETUPTIME_HI = <time value>
If either of the time values is 0, then no check is done for that
case.
HOLDTIME is used in the same way as SETUPTIME and also
has the alternate _LH and _HL formats and 0 value condition.
RELEASETIME causes the simulator to perform a
special-purpose setup check. Release time (also referred to
as recovery time in some data sheets) refers to the minimum
time that a signal can go inactive before the active clock edge.
Again, the _LH and _HL forms are available. The difference
between RELEASETIME and SETUPTIME checking is that
simultaneous CLOCK/DATA transitions are never allowed
(this assumes a nonzero hold time). RELEASETIME is usually
not used in conjunction with SETUPTIME or HOLDTIME.
Width
WIDTH does the minimum pulse-width checking. MIN_HI/
MIN_LO is the minimum time that the node can remain
HI/LOW. The value must be a nonnegative constant, or
PSpice User's Guide
365
Chapter 7
Digital device modeling
Product Version 10.5
expression. A value of 0 means that any pulse width is
allowed. At least one of MIN_HI or MIN_LO must be used
within a WIDTH section.
Freq
FREQ checks the frequency. MINFREQ/MAXFREQ is the
minimum/maximum frequency that is allowed on the node in
question. The value must be a nonnegative floating point
constant or expression measured in hertz. At least one of
MINFREQ or MAXFREQ must be used within a FREQ
section.
AFFECTS clauses (not used in this example) can be included
in constraints to describe how the simulator should associate
the failure of a constraint check with the outputs (paths
through the device) of the PINDLY. This information does not
affect the logic state of the outputs but provides causality
detail used by the error tracking mechanism in PSpice A/D
waveform analysis.
74160 example
In the 74160 example, we are checking that the maximum
clock frequency (CLK) is not more than 25 MHz and the pulse
width is 25 ns. We are also checking that the CLRBAR signal
has a minimum LO pulse width of 20 ns, and that the 4 data
inputs (A, B, C, D) have a setup/hold time of 20 ns in reference
to the CLK signal. We are also checking that ENP and ENT
have a setup/hold time of 20 ns with respect to the 0 to 1
transition of the CLK signal, but only when the conditions in
the WHEN statement are met. All of the delay and constraint
checking values were taken directly from the actual data
sheet. This makes the delay modeling both easy and
accurate.
All of the above primitives and modeling methods, as well as
a few special cases that are not covered here, can be found in
the Digital Devices chapter of the online PSpice Reference
Guide.
* 74160 Synchronous 4-bit Decade Counters with asynchronous clear
366
PSpice User's Guide
Product Version 10.5
Chapter overview
* Modeled using LOGICEXP, PINDLY, & CONSTRAINT devices
.SUBCKT 74160 CLK_I ENP_I ENT_I CLRBAR_I LOADBAR_I A_I B_I C_I D_I
+ QA_O QB_O QC_O QD_O RCO_O
+ OPTIONAL: DPWR=$G_DPWR DGND=$G_DGND
+ PARAMS: MNTYMXDLY=0 IO_LEVEL=0
*
U160LOG LOGICEXP(14,20) DPWR DGND
+ CLK_I ENP_I ENT_I CLRBAR_I LOADBAR_I A_I B_I C_I D_I
+ QDBAR QA QB QC QD
+ CLK ENP ENT CLRBAR LOADBAR A B C D
+ CLKBAR RCO JA JB JC JD KA KB KC KD EN
+ D0_GATE IO_STD IO_LEVEL={IO_LEVEL}
+ LOGIC:
+ CLK = { CLK_I }
;Buffering
+ ENP = { ENP_I }
+ ENT = { ENT_I }
+ CLRBAR = { CLRBAR_I }
+ LOADBAR = { LOADBAR_I }
+ A = { A_I }
+ B = { B_I }
+ C = { C_I }
+ D = { D_I }
+ CLKBAR = { ~CLK }
;Logic expressions
+ LOAD = { ~LOADBAR }
+ EN = { ENP & ENT }
+ I1A = { LOAD | EN }
+ I2A = { ~(LOAD & A) }
+ JA = { I1A & ~(LOAD & I2A) }
+ KA = { I1A & I2A }
+ I1B = { (QA & EN & QDBAR) | LOAD }
+ I2B = { ~(LOAD & B) }
+ JB = { I1B & ~(LOAD & I2B) }
+ KB = { I1B & I2B }
+ I1C = { (QA & EN & QB) | LOAD }
+ I2C = { ~(LOAD & C) }
+ JC = { I1C & ~(LOAD & I2C) }
+ KC = { I1C & I2C }
+ I1D = { ((QC & QB & QA & EN) | (EN & QA & QD)) | LOAD }
+ I2D = { ~(LOAD & D) }
+ JD = { I1D & ~(LOAD & I2D) }
+ KD = { I1D & I2D }
+ RCO = { QD & QA & ENT }
*
UJKFF JKFF(4) DPWR DGND $D_HI CLRBAR CLKBAR JA JB JC JD KA KB KC KD
+ QA QB QC QD QABAR QBBAR QCBAR QDBAR D0_EFF IO_STD
U160DLY PINDLY (5,0,10) DPWR DGND
+ RCO QA QB QC QD
+ CLK LOADBAR ENT CLRBAR ENP A B C D EN
+ RCO_O QA_O QB_O QC_O QD_O
+ IO_STD MNTYMXDLY={MNTYMXDLY} IO_LEVEL={IO_LEVEL}
+ BOOLEAN:
+ CLOCK = { CHANGED_LH(CLK,0) }
+ CNTENT = { CHANGED(ENT,0) }
+ PINDLY:
+ QA_O QB_O QC_O QD_O = {
+ CASE(
+ CLOCK & LOADBAR=='1 & TRN_LH, DELAY(-1,13NS,20NS),
+ CLOCK & LOADBAR=='1 & TRN_HL, DELAY(-1,15NS,23NS),
+ CLOCK & LOADBAR=='0 & TRN_LH, DELAY(-1,17NS,25NS),
PSpice User's Guide
367
Chapter 7
Digital device modeling
Product Version 10.5
+ CLOCK & LOADBAR=='0 & TRN_HL, DELAY(-1,19NS,29NS),
+ CHANGED_HL(CLRBAR,0), DELAY(-1,26NS,38NS),
+ DELAY(-1,26NS,38NS)
+
)
+ }
+ RCO_O = {
+ CASE(
+ CNTENT, DELAY(-1,11NS,16NS),
+ CLOCK, DELAY(-1,23NS,35NS),
+ DELAY(-1,23NS,35NS)
+ )
+ }
+ FREQ:
+ NODE = CLK
+ MAXFREQ = 25MEG
+ WIDTH:
+ NODE = CLK
+ MIN_LO = 25NS
+ MIN_HI = 25NS
+ WIDTH:
+ NODE = CLRBAR
+ MIN_LO = 20NS
+ SETUP_HOLD:
+ DATA(4) = A B C D
+ CLOCK LH = CLK
+ SETUPTIME = 20NS
+ WHEN = { (LOADBAR!='1 ^ CHANGED(LOADBAR,0)) &
+
CLRBAR!='0 }
+ SETUP_HOLD:
+ DATA(2) = ENP ENT
+ CLOCK LH = CLK
+ SETUPTIME = 20NS
+ WHEN = { CLRBAR!='0 & (LOADBAR!='0 ^
+
CHANGED(LOADBAR,0))
+ & CHANGED(EN,20NS) }
+ SETUP_HOLD:
+ DATA(1) = LOADBAR
+ CLOCK LH = CLK
+ SETUPTIME = 25NS
+ WHEN = { CLRBAR!='0 }
+ SETUP_HOLD:
+ DATA(1) = CLRBAR
+ CLOCK LH = CLK
+ RELEASETIME_LH = 20NS
.ENDS
368
PSpice User's Guide
Part three: Setting up and
running analyses
Part Three describes how to set up and run analyses and
provides setup information specific to each analysis type.
PSpice User's Guide
■
Chapter 8, “Setting up analyses and starting simulation,”
explains the procedures general to all analysis types to
set up and start the simulation.
■
Chapter 9, “DC analyses,” describes how to set up DC
analyses, including DC sweep, bias point detail,
small-signal DC transfer, and DC sensitivity.
■
Chapter 10, “AC analyses,” describes how to set up AC
sweep and noise analyses.
■
Chapter 12, “Overview of transient analysis,” describes
how to set up transient analysis and optionally Fourier
components. This chapter also explains how to use the
Stimulus Editor to create time-based input.
■
Chapter 11, “Parametric and temperature analysis,”
describes how to set up parametric and temperature
analyses, and how to run post-simulation performance
analysis in Probe on the results of these analyses.
■
Chapter 13, “Monte Carlo and sensitivity/worst-case
analyses,” describes how to set up Monte Carlo and
sensitivity/worst-case analyses for statistical
interpretation of your circuit’s behavior.
369
Chapter
370
Part three: Setting up and running analyses
Product Version 10.5
■
Chapter 14, “Digital simulation,” describes how to set up
a digital simulation analysis on either a digital-only or
mixed-signal circuit.
■
Chapter 15, “Mixed analog/digital simulation,” explains
how PSpice A/D processes the analog and digital
interfaces in mixed-signal circuits.
■
Chapter 16, “Digital worst-case timing analysis,”
describes how PSpice A/D performs digital worst-case
timing analysis and the kinds of hazards that this analysis
can help you detect.
PSpice User's Guide
Setting up analyses and starting
simulation
8
Chapter overview
This chapter provides an overview of setting up analyses and
starting simulation that applies to any analysis type. The other
chapters in Part three: Setting up and running analyses
provide specific analysis setup information for each analysis
type.
This chapter includes the following sections:
PSpice User's Guide
■
Analysis types on page 372
■
Setting up analyses on page 373
■
Performance package on page 383
■
Starting a simulation on page 385
■
Interacting with a simulation
■
Using the Simulation Manager
371
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Analysis types
PSpice supports analyses that can simulate analog-only,
mixed-signal, and digital-only circuits.
PSpice fully supports digital analysis by simulating the timing
behavior of digital devices within a standard transient analysis,
including worst-case (min/max) timing. For mixed
analog/digital circuits, all of the above-mentioned analyses
can be run. If the circuit is digital-only, only the transient
analysis can be run.
Table 8-1 provides a summary of the available PSpice
analyses and the corresponding Analysis type options where
the analysis parameters are specified. In Capture, switch to
the PSpice view, then from the PSpice menu, choose New
Simulation Profile.
Table 8-1 Classes of PSpice analyses
Analysis
Analysis type or Swept
Option
variable
Standard analyses
DC sweep
DC Sweep
source
parameter
temperature
Bias point
Bias Point
Small-signal DC transfer
Bias Point
DC sensitivity
Bias Point
Frequency response
AC Sweep/Noise frequency
Noise (requires a frequency AC Sweep/Noise frequency
response analysis)
372
Transient response
Time Domain
(Transient)
time
Fourier (requires transient
response analysis)
Time Domain
(Transient)
time
PSpice User's Guide
Product Version 10.5
Setting up analyses
Table 8-1 Classes of PSpice analyses, continued
Analysis
Analysis type or Swept
Option
variable
Simple multi-run analyses
Parametric1
Parametric
Sweep
Temperature
Temperature
(Sweep)
Statistical analyses
Monte Carlo2
Monte Carlo/
Worst Case
Sensitivity/worst-case3
Monte Carlo/
Worst Case
1. Parametric analysis is not included in PSpice A/D Basics.
2. Monte Carlo analysis is not included in PSpice A/D Basics.
3. Sensitivity/worst-case analysis is not included in PSpice A/D
Basics.
The waveform analyzer calculates and displays the results of
PSpice simulations for swept analyses. The waveform
analyzer also generates supplementary analysis information
in the form of lists and tables, and saves this in the simulation
output file.
See Part four: Viewing results, for information about using
waveform analysis in PSpice.
Setting up analyses
Specific information for setting up each type of analysis is
discussed in the following chapters.
To set up one or more analyses
PSpice User's Guide
1
From the PSpice menu, choose New Simulation Profile.
2
Enter the name of the profile and click Create.
373
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
3
Click the Analysis tab if it is not already the active tab in
the dialog box.
4
Enter the necessary parameter values and select the
appropriate check boxes to complete the analysis
specifications.
See Output variables on page 376 for a description of the
output variables that can be entered in the Simulation
Settings dialog box displayed for an analysis type.
5
Set up any other analyses you want to perform for the
circuit by selecting any of the remaining analysis types
and options, then complete their setup dialog boxes.
Specific information for setting up each type of analysis is
discussed in the following chapters.
Execution order for standard analyses
For normal simulations that are run from a simulation profile,
or in batch mode, only the particular analysis type that is
specified will be executed.
During simulation of a circuit file, the analysis types are
performed in the order shown in Table 8-2. Each type of
analysis is conducted only once per run.
374
PSpice User's Guide
Product Version 10.5
Setting up analyses
Several of the analyses (small-signal transfer, DC sensitivity,
and frequency response) depend upon the bias point
calculation. Because so many analyses use the bias point,
PSpice calculates this automatically. PSpice’s bias point
calculation computes initial states of digital components as
well as the analog components.
.
Table 8-2 Execution order for standard analysis
1. DC sweep
2. Bias point
3. Frequency response
4. Noise
5. DC sensitivity
6. Small-signal DC transfer
7. Transient response
8. Fourier components
PSpice User's Guide
375
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Output variables
Certain analyses (such as noise, Monte Carlo, sensitivity/
worst-case, DC sensitivity, Fourier, and small-signal DC
transfer function) require you to specify output variables for
voltages and currents at specific points on the schematic.
Depending upon the analysis type, you may need to specify
the following:
■
Voltage on a net, a pin, or at a terminal of a
semiconductor device
■
Current through a part or into a terminal of a
semiconductor device
■
A device name
If output variables or other information are required, select
Output File Options in the Monte Carlo/Worst Case dialog box
and enter the required parameters.
Voltage
Specify voltage in the following format:
v[modifiers](<out id>[,<out id>])
(1)
where <out id > is:
<net id> or <pin id>
(2)
<net id> is a fully qualified net name
(3)
<pin id> is <fully qualified device
name>:<pin name>
(4)
A fully qualified net name (as referred to in line 3 above) is
formed by prefixing the visible net name (from a label applied
to one of the segments of a wire or bus, or an offpage port
connected to the net) with the full hierarchical path, separated
by periods. At the top level of hierarchy, this is just the visible
name.
A fully qualified device name (from line 4 above) is
distinguished by specifying the full hierarchical path followed
376
PSpice User's Guide
Product Version 10.5
Setting up analyses
by the device’s part reference, separated by period
characters. For example, a resistor with part reference R34
inside part Y1 placed on a top-level schematic page is referred
to as Y1.R34 when used in an output variable.
A <pin id> (from line 4) is uniquely distinguished by specifying
the full part name (as described above) followed by a colon,
and the pin name. For example, the pins on a capacitor with
reference designator C31 placed on a top-level page and pin
names 1 and 2 would be identified as C31:1 and C31:2,
respectively.
Current
Specify current in the following format:
i[modifiers](<out device>[:modifiers])
where <out device> is a fully qualified device name.
Modifiers
The basic syntax for output variables can be modified to
indicate terminals of semiconductors and AC specifications.
The modifiers come before <out id> or <out device>. Or,
when specifying terminals (such as source or drain), the
modifier is the pin name contained in <out id>, or is appended
to <out device> separated by a colon.
Modifiers can be specified as follows:
■
For voltage:
v[AC suffix](<out id>[, out id])
v[terminal]*(<out device>)
■
For current:
i[AC suffix](<out device>[:terminal])
i[terminal][AC suffix](<out device>])
PSpice User's Guide
377
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
where
terminal
AC suffix
out id
out device
specifies one or two terminals for
devices with more than two terminals,
such as D (drain), G (gate), S (source)
specifies the quantity to be reported
for an AC analysis, such as M
(magnitude), P (phase), G (group
delay)
specifies either the <net id> or <pin
id> (<fully qualified device
name>:<pin name>)
specifies the <fully qualified device
name>
These building blocks can be used for specifying output
variables as shown in Table 8-3 (which summarizes the
accepted output variable formats) and Tables 8-4 through 8-7
(which list valid elements for two-terminal, three- or
378
PSpice User's Guide
Product Version 10.5
Setting up analyses
four-terminal devices, transmission line devices, and AC
specifications).
Table 8-3 PSpice output variable formats
Format
Meaning
V[ac ](< + out id >)
voltage at out id
V[ac ](< +out id >,< - out id >)
voltage across + and out id’s
V[ac ](< 2-terminal device out id >) voltage at a 2-terminal
device out id
V[ac ](< 3 or 4-terminal device out voltage at non-grounded
id >) or
terminal x of a
3 or 4-terminal device
V<x >[ac ](< 3 or 4-terminal out
device >)
V<x ><y >[ac ](< 3 or 4-terminal out voltage across terminals
device >)
x and y of a
3 or 4-terminal device
V[ac ](< transmission line out id >) voltage at one end z of
or
a transmission line
V<z >[ac ](< transmission line out
device >)
device
I[ac ](< 3 or 4-terminal out device
>:<x >) or
current through
non-grounded terminal
x of a 3 or 4-terminal
I<x >[ac ](< 3 or 4-terminal out
device >)
PSpice User's Guide
out device
I[ac ](< transmission line out
device >:<z >) or
current through one end
z of a transmission line
I<z >[ac ](< 3 or 4-terminal out
device >)
out device
< DC sweep variable >
voltage or current
source name
379
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Table 8-4 Element definitions for 2-terminal devices
Device type
< out id > or
< out device >
device
indicator
Output variable
examples
capacitor
C
V(CAP:1)
I(CAP)
diode
D
V(D23:1)
I(D23)
voltage-controlled
voltage source
E
current-controlled
current source
F
voltage-controlled
current source
G
current-controlled
voltage source
H
independent
current source
I
inductor
L
V(E14:1)
I(E14)
V(F1:1)
I(F1)
V(G2:1)
I(G2)
V(HSOURCE:1)
I(HSOURCE)
V(IDRIV:+)
I(IDRIV)
V(L1:1)
I(L1)
resistor
R
V(RC1:1)
I(RC1)
380
voltage-controlled
switch
S
independent
voltage source
V
current-controlled
switch
W
V(SWITCH:+)
I(SWITCH)
V(VSRC:+)
I(VSRC)
V(W22:-)
I(W22)
PSpice User's Guide
Product Version 10.5
Setting up analyses
Table 8-5 Element definitions for 3- or 4-terminal devices
Device type
< out id >
or
< out
device >
device
indicator
GaAs MESFET B
< pin id >
Output
variable
examples
D (Drain terminal)
V(B11:D)
G (Gate terminal)
ID(B11)
S (Source terminal)
Junction FET
J
D (Drain terminal)
VG(JFET)
G (Gate terminal)
I(JFET:G)
S (Source terminal)
MOSFET
M
B (Bulk, substrate
terminal)
VDG(M1)
ID(M1)
D (Drain terminal)
G (Gate terminal)
S (Source terminal)
bipolar
transistor
Q
B (Base terminal)
V(Q1:B)
C (Collector terminal) I(Q1:C)
E (Emitter terminal)
S (Source terminal)
IGBT
Z
C (Collector terminal) V(Z1:C)
E (Emitter terminal)
I(Z1:C)
G (Gate terminal)
PSpice User's Guide
381
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Table 8-6 Element definitions for transmission line
devices
Device type
<z >
< out id > or
< out device >
device
indicator
Output
variable
examples
transmission
line
T
A (Port A)
V(T32:A+)
B (Port B)
I(T32:B-)
Table 8-7 Element definitions for AC analysis specific
elements
<ac suffix >
device
symbol
Meaning
Output variable
examples
(none)
magnitude (default)
V(V1)
I(V1)
M
magnitude
VM(CAP1:1)
IM(CAP1:1)
DB
magnitude in decibels VDB(R1)
P
phase
IP(R1)
R
real part
VR(R1)
I
imaginary part
VI(R1)
The INOISE, ONOISE, DB(INOISE), and DB(ONOISE) output
variables are predefined for use with noise (AC sweep)
analysis.
382
PSpice User's Guide
Product Version 10.5
Setting up analyses
Performance package
PSpice includes two solution algorithms: Solver 0 and
Solver 1.
Note: The Performance package is not included in PSpice
A/D Basics.
To choose a solver setting
1
From the Capture PSpice menu, choose Edit Simulation
Profile.
or
From the PSpice Simulation menu, choose Edit Profile.
The Simulation Settings dialog box appears.
2
Click the Options tab, then click the Advanced Options
button.
The Advanced Analog Options dialog box appears.
3
In the Simulation algorithm drop-down list, select one of
the following choices:
❑
0 - the PSpice simulation engine uses the original
PSpice solution algorithm.
❑
1 - the PSpice simulation engine uses an advanced
solution algorithm that provides significant speed
improvements.
Solver 1 is particularly useful for larger MOS and
bipolar circuits with substantial runtimes.
PSpice User's Guide
383
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Note: Solver 1 is not available with PSpice A/D
Basics.
❑
Default - the PSpice simulation engine internally
chooses Solver 0 or 1 based on the installed
software.
The default for the PSpice A/D Basics package is
Solver 0. For all other PSpice configurations the
default is Solver 1.
Note: If Solver 1 is selected with the PSpice A/D Basics
package, an error message will occur during simulation
stating that the requested solver is not available. To fix the
problem, change the solver setting to default or 0.
4
Click OK to close the Advanced Analog Options dialog
box.
5
Click OK to close the Options dialog box.
See the online PSpice Reference Guide for .OPTIONS
statements that use SOLVER to specify a solution algorithm.
384
PSpice User's Guide
Product Version 10.5
Setting up analyses
Starting a simulation
After you have used Capture to enter your circuit design and
have set up the analyses to be performed, you can start a
simulation by choosing Run from the PSpice menu. When you
enter and set up your circuit this way, Capture automatically
generates the simulation files and starts PSpice.
There may be situations, however, when you want to run
PSpice outside of Capture. You may want to simulate a circuit
that was not created in Capture, for example, or you may want
to run simulations of multiple circuits in batch mode.
This section includes the following:
■
Creating a simulation netlist on page 385
■
Starting a simulation from Capture on page 394
■
Starting a simulation outside of Capture on page 394
■
Setting up batch simulations on page 395
■
The PSpice simulation window on page 396
Creating a simulation netlist
A netlist is the connectivity description of a circuit, showing all
of the components, their interconnections, and their values.
When you create a simulation netlist from OrCAD Capture,
that netlist describes the current design.
You have a choice between two types of netlist formats:
■
a flat netlist
■
a hierarchical netlist
The flat netlist is generated for all levels of hierarchy, starting
from the top, regardless of whether you are pushed into any
level of the hierarchy. Flat netlists are most commonly used as
input to PCB layout tools. The flat simulation netlist format for
PSpice contains device entries for all parts on a subcircuit
(child) schematic multiple times, once for each instance of the
hierarchical part or block used.
PSpice User's Guide
385
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
The hierarchical netlist preserves the hierarchical information
in any subcircuit (child) schematics. It contains a single
.SUBCKT definition for each child schematic. The devices in
the subcircuit are therefore netlisted only once. Each instance
of the hierarchical part or block is then netlisted as an instance
of that subcircuit (as an “X” device). The subcircuit name
corresponds to the name of the subcircuit (child) schematic.
Hierarchical netlists are especially useful to IC designers who
want to perform Layout vs. Schematic (LVS) verification
because they are more accurate descriptions of the true
circuit. The hierarchical netlist format supports LVS tools such
as Dracula.
Using netlisting templates
In OrCAD Capture, the PSPICETEMPLATE property specifies
how primitive parts are described in the simulation netlist. It
defines the pin order and which other part property values to
include in the netlist. Only parts with a PSPICETEMPLATE
property are included in the simulation. In the process of
creating the netlist, buses, connectors, and so on, are
resolved.
An alternate template option is provided which allows you to
define which netlisting template property to use. This option
applies to both flat and hierarchical netlists. With this option,
you may specify a particular netlist template for generating
netlists that can be used by other simulation tools, for
example, or for creating alternate PSpice netlists that contain
different part descriptions.
To learn more about using alternate netlist templates, see
Specifying alternate netlist templates on page 393.
Passing parameters to subcircuits
Hierarchical netlists have the advantage of allowing
parameters to be passed from the top level schematic to any
subcircuit schematics. To take advantage of this feature, you
must use the new SUBPARAM part in the SPECIAL.OLB
library.
386
PSpice User's Guide
Product Version 10.5
Setting up analyses
Note: Hierarchical netlists do not support cross-probing from
a subcircuit, nor do they support probe markers in a
subcircuit.
With the SUBPARAM part, you can pass parameters from the
top-level schematic to a subcircuit schematic. This allows you
to explicitly define the properties and default values to be used
during netlisting and simulation.
To set up parameter passing to a subcircuit using
SUBPARAM
1
Make the subcircuit your active schematic page in the
Capture editor.
2
From the Place menu, choose the Part command.
3
Select the part SUBPARAM from the PSpice library
SPECIAL.OLB and place it on the subcircuit.
4
With the SUBPARAM part still selected, from the Edit
menu, choose Properties.
The Property Editor spreadsheet appears.
5
In the spreadsheet, define the names and default values
for the properties that can be changed on an
instance-by-instance basis.
6
In the top-level schematic, use the Property Editor
spreadsheet to edit the properties of the hierarchical part
or block that references the subcircuit (child) schematic
so they match the properties you defined in Step 5.
Any part in the subcircuit (child) schematic can reference the
properties in its PSPICETEMPLATE. The PSpice subcircuit
mechanism supports parameterizing:
PSpice User's Guide
■
constants specified on device statements
■
model parameters
■
expressions consisting of constants
■
parameters
■
functions
387
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Creating the netlist
You can generate a simulation netlist in one of two ways:
■
from Capture’s Project Manager by using the Create
Netlist command under the Tools menu. (If this is the first
time you’re creating a hierarchical netlist for this project,
you can only use this method.)
- or -
■
directly from within Capture itself by using the Create
Netlist command under the PSpice menu.
During the netlist process, Capture creates several files with
different extensions: the .NET file contains the netlist; the .CIR
file contains simulation commands; and the .ALS file contains
alias information.
To create a flat netlist
1
In the Capture Project manager, select the design file
(.DSN) you want to netlist.
2
From the Tools menu, choose Create Netlist to display the
Create Netlist dialog box.
3
Select the PSpice tab.
4
Under the Options frame, leave all the check boxes blank.
5
In the Netlist File text box, type a name for the output file,
or click the Browse button to assign a filename.
6
If desired, click the View Output check box to display the
netlist after it has been generated.
7
Click OK.
To create a hierarchical netlist
1
388
In the Capture Project manager, select the design file
(.DSN) you want to netlist.
PSpice User's Guide
Product Version 10.5
Setting up analyses
2
From the Tools menu, choose Create Netlist to display the
Create Netlist dialog box.
3
Select the PSpice tab.
4
Under the Options frame, click Create Hierarchical
Format Netlist.
5
Click Settings to customize the format of the hierarchical
netlist (see Customizing the hierarchical netlist on
page 390).
6
Click Create Subcircuit Format Netlist to specify how
subcircuits will be netlisted (see Creating subcircuit
netlists on page 392).
7
In the Use Template list box, select the netlisting
template(s) you wish to apply (see Specifying alternate
netlist templates on page 393).
8
In the Netlist File text box, type a name for the output file,
or click the Browse button to assign a filename.
9
If desired, click the View Output check box to display the
netlist after it has been generated.
10 Click OK.
PSpice User's Guide
389
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
For more information on netlist formats, refer to OrCAD
Capture’s online help.
Customizing the hierarchical netlist
You can customize the hierarchical netlist by specifying
various options using the Settings button in the Create Netlist
dialog box. You can also customize the format of the subcircuit
definition and reference text in the netlist. These settings,
once defined, will apply to all subsequent PSpice netlists
whether the netlist is invoked from the Tools menu in the
Project Manager or directly from the schematic editor.
Two groups of settings are saved: PSpice and LVS. Having
two groups makes it easy to switch between netlisting for
PSpice and netlisting for an LVS compatible format. You can
specify which group of settings is active for the netlister by
using the Products list box.
Note: The settings you define are project specific. If you want
to save the settings globally, click the Save as Default
Project Settings button.
390
PSpice User's Guide
Product Version 10.5
Setting up analyses
To customize the hierarchical netlist
1
In the PSpice tab of the Create Netlist dialog box, under
the Options frame, click Create Hierarchical Format
Netlist.
2
Click Settings, then enable or specify the following
options, as desired:
❑
Make .PARAM Commands Global: If this check box
is enabled, any param parts in the design become
global in scope. If it is disabled, the param parts are
local to the subcircuit in which they occur.
❑
Products: This list box specifies which group of
settings is active for the netlister. Selecting a different
group changes the Subcircuit Patterns frame to
reflect the settings of the specified tool.
❑
Global Net Prefix: This text box allows you to define
the syntax of the global net of a subcircuit.
❑
Reference frame
❍
PSpice User's Guide
Subcircuit Call: This list box allows you to select
the syntax of the subcircuit call using a modified
TEMPLATE syntax.
391
Chapter 8
Setting up analyses and starting simulation
❍
❑
❑
3
Product Version 10.5
ParamList Element Definition: This list box
allows you to select the syntax of how
parameters are passed from a reference to a
part definition.
Definition frame
❍
Subcircuit Header: This list box allows you to
select the syntax of the subcircuit header using
a modified TEMPLATE syntax. If modified, you
must make sure the definition header is
consistent with the call.
❍
ParamList Element Definition: This list box
allows you to select the syntax of how
parameters are passed from a reference to a
part definition.
❍
Param Usage Reference: This list box allows
you to select the syntax used to enclose the
parameters in references.
❍
Subcircuit Ends: This list box allows you to
select the syntax used for the termination of a
subcircuit.
Save as Project Default Settings: This button saves
the current settings in the CAPTURE.INI file, and
thereby makes the current settings the default
settings for any new Capture projects.
Click OK.
For more detailed information about the syntax for these
commands, and examples of how to use them, see the online
PSpice Reference Guide.
Creating subcircuit netlists
You can specify how subcircuits in a hierarchical design are
processed and defined in the simulation netlist.
392
PSpice User's Guide
Product Version 10.5
Setting up analyses
To create a subcircuit format netlist
1
In the Capture Project manager, select the design file
(.DSN) you want to netlist.
2
From the Tools menu, choose Create Netlist to display the
Create Netlist dialog box.
3
Select the PSpice tab.
4
Under the Options frame, click Create Subcircuit Format
Netlist, then click one of the following options, as desired:
❑
Descend: This generates a definition of a
hierarchical design that includes the top level circuit
as well as its subcircuits. (This option is only
available if Create Hierarchical Format Netlist is
enabled.)
❑
Do Not Descend: This generates a definition of a
hierarchical design that includes only the top level
circuit, without any of its subcircuits. (This option is
only available if Create Hierarchical Format Netlist is
enabled.)
❑
Descend and Fully Expand: This generates a
definition of a flat design. (This option is only
available if Create Hierarchical Format Netlist is not
enabled.)
Specifying alternate netlist templates
To specify an alternate netlist template
PSpice User's Guide
1
In the Capture Project manager, select the design file
(.DSN) you want to netlist.
2
From the Tools menu, choose Create Netlist to display the
Create Netlist dialog box.
3
Select the PSpice tab.
4
In the Use Template list box, select the name of the
template you want to use.
393
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
By default, the netlister will use the PSPICETEMPLATE.
Alternate templates in the Use Template list box will be
processed in the order in which they appear. The ordering of
the templates is therefore important to the netlister and
determines what the output will be.
Use the control buttons located directly above the Use
Template list box to configure the list of templates. You can:
■
Add a new template by clicking the New icon or by
double-clicking in the dashed box at the beginning of the
list.
■
Delete a template by selecting the name and then clicking
the Delete icon.
■
Edit a template name by selecting the name and then
clicking the Edit icon.
■
Change the order of the listing (move a template up or
down in the listing) by selecting the name and clicking the
Up or Down arrows.
Note: Templates are not specific to either a flat or hierarchical
netlist. The same template may be used for both types.
Starting a simulation from Capture
After you have set up the analyses for the circuit, you can start
a simulation from Capture in either of the following ways:
■
From the PSpice menu select Run.
■
Click the Simulate button
on the PSpice toolbar.
Starting a simulation outside of Capture
To start PSpice outside of Capture
394
1
From the Start menu, point to the Release OrCAD 10.0
program group, then choose PSpice.
2
From the File menu, choose Open Simulation.
PSpice User's Guide
Product Version 10.5
Setting up analyses
3
Do one of the following:
❑
Double-click on the simulation profile filename
(*.SIM) in the list box.
❑
Enter the simulation profile filename (*.SIM) in the
File name text box and click Open.
4
From the Simulation menu, choose Edit Settings to
modify any of the analysis setup parameters.
5
From the Simulation menu, choose Run (or click the Run
toolbar button) to begin the simulation.
Setting up batch simulations
Multiple simulations can be run in batch mode when starting
PSpice directly with circuit file input. You can use batch mode,
for example, to run a number of simulations overnight. There
are two ways to do this, as described below.
Multiple simulation setups within one circuit file
Multiple circuit/simulation descriptions can be concatenated
into a single circuit file and simulated all at once with PSpice.
Each circuit/simulation description in the file must begin with
a title line and end with a .END statement.
The simulator reads all the circuits in the circuit file and then
processes each one in sequence. The data file and simulation
output file contain the outputs from each circuit in the same
order as they appeared in the circuit file. The effect is the
same as if you had run each circuit separately and then
concatenated all of the outputs.
Running simulations with multiple circuit files
You can direct PSpice to simulate multiple circuit files using
either of the following methods.
PSpice User's Guide
395
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Method 1
1
From the Start menu, point to the Release OrCAD 10.0
program group, then choose PSpice.
2
Select Open Simulation from the File menu from the
PSpice window.
3
Do one of the following:
❑
Type each file name enclosed in double quotation
marks in the File Name text box separated by a
space.
❑
Use the combination keystrokes and mouse clicks in
the list box as follows: Ctrl+click to select file names
one at a time, and Shift+click to select groups of
files.
Method 2
1
From the Start menu, point to the Release OrCAD 10.0
program group, then choose PSpice.
2
Update the command line in the following way:
❑
Include a list of circuit file names separated by
spaces.
Circuit file names can be fully qualified or can contain the
wild card characters (* and ?).
The PSpice simulation window
The PSpice Simulation Window is an MDI (Multiple Document
Interface) application. This implies that you can open and
display multiple files at the same time in this window. For
instance, you can have a waveform file (.DAT), a circuit file
(.CIR), and a simulation output file (.OUT) open and displayed
in different child windows within this one window.
The PSpice Simulation Window consists of three sections: the
main window section where the open files are displayed, the
output window section where output information such as
informational, warning, and error messages from the
396
PSpice User's Guide
Product Version 10.5
Setting up analyses
simulator are shown, and the simulation status window
section where detailed status information about the simulation
are shown. These three sections are shown in Figure 8-1.
The windows in these sections may be resized, moved, and
reordered as needed.
The simulation window also includes a menu bar and toolbars
for controlling the simulation and the waveform display.
Title bar
The title bar of the simulation window (the area at the top of
the window) identifies the name of the currently open
simulation (either simulation profile or circuit file) and the
name of the currently active document displayed in the main
window area. For example, the simulation window shown in
Figure 8-1 indicates that simulation profile Example-TRAN is
currently open and the active document displayed is
Example-Example-TRAN.DAT.
Menus and Toolbars
The menus accessed from the menu bar include commands
to set up and control the simulator, customize the window
display characteristics, and configure the way the waveforms
PSpice User's Guide
397
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
are displayed. The toolbar buttons duplicate many of the more
frequently used commands.
Figure 8-1 PSpice simulation window
Main window section
The top central portion (by default) of the simulation window is
the main window section where documents (such as
waveforms, circuit description, output information etc.) are
displayed within child windows. These windows are tabbed by
default. The tabs at the bottom left show the names of the
documents that each child window contains. Clicking on a tab
brings that child window to the foreground. Figure 8-1 shows
the tabbed document windows for
Example-Example-TRAN.DAT and
Example-Example-TRAN.OUT.
You can configure the display of these windows to suit your
preferences and to make the analysis of the circuit quick and
readily understandable. These windows can also be resized,
moved, and reordered to suit your needs.
398
PSpice User's Guide
Product Version 10.5
Setting up analyses
Output window section
The lower left portion of the simulation window provides a
listing of the output from the simulation. It shows informational,
warning, and error messages from the simulation. You can
resize and relocate this window to make it easier to read.
Simulation status window section
The lower right portion of the simulation window presents a set
of tabbed windows that show detailed status about the
simulation. There are three tabbed windows in this section:
the Analysis window, the Watch Variable window, and the
Devices window. The Analysis window provides a running log
of values of simulation variables (parameters such as
Temperature, Time Step, and Time). The Watch Variable
window displays watch variables and their values. These are
the variables setup to be monitored during simulation. The
Devices window displays the devices that are being simulated.
PSpice User's Guide
399
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Interacting with a simulation
PSpice includes options for interacting with a simulation by
changing certain runtime parameters in the course of the
analysis. With the interactive simulation feature, you can do
the following:
■
Extend a transient analysis after TSTOP has been
reached in order to achieve the desired results.
■
Interrupt a bias or transient analysis, change certain
runtime parameters, and then resume the simulation with
the new settings.
■
Schedule changes to certain runtime parameters so that
they are made automatically during a simulation.
Note: The ability to interact with a simulation only applies to
bias point and transient analyses. You cannot interact
with other analysis types.
What the various versions of PSpice support
The following table identifies what interactive functionality is
available with each version of PSpice.
PSpice version
Interactive simulation
functionality
PSpice Lite
Extend transient analysis
PSpice A/D Basics
PSpice
Extend transient analysis
PSpice A/D
Interrupt a simulation, change
parameters, and resume the
simulation
Schedule automatic changes to
parameters during simulation
400
PSpice User's Guide
Product Version 10.5
Setting up analyses
Extending a transient analysis
Often, a long transient analysis will run to the completion time
(TSTOP) without achieving the desired simulation results
(achieving a steady state, for instance). To achieve better
results, the value for TSTOP would have to be increased and
the entire simulation would have to be rerun from the
beginning. This was time-consuming and inefficient for large
simulations.
A transient analysis will automatically pause rather than stop
when it reaches the TSTOP value. Once paused, you can
review the results and determine if the simulation should run
longer. If desired, you can increase the value of TSTOP and
resume the transient analysis from the point at which it
paused, thus saving a good deal of processing time.
Note: For more details about using TSTOP, see the online
PSpice Reference Guide.
To help clarify under what conditions simulations will either be
terminated or paused, the following table explains the different
behaviors of PSpice for particular simulation scenarios:
PSpice User's Guide
Simulation scenario
Behavior of PSpice
Running a single transient
simulation using a profile
or a circuit file containing
one circuit.
PSpice will pause after a
successful simulation, or if a
convergence error occurs,
allowing you to change certain
runtime parameters and
resume the analysis.
Running a single AC/DC
simulation using a profile
or a circuit file containing
one circuit.
PSpice will stop (terminate)
after a successful simulation.
-orPSpice will pause if a
convergence error occurs,
allowing you to change certain
runtime parameters and
resume the analysis.
401
Chapter 8
Setting up analyses and starting simulation
Simulation scenario
Product Version 10.5
Behavior of PSpice
Running a single
PSpice will stop (terminate)
simulation with a profile or after a successful simulation, or
a circuit file containing
if a convergence error occurs.
outer loops.
Running a queued
simulation.
PSpice will stop (terminate)
after a successful simulation, or
if a convergence error occurs.
Launching a new
simulation when another
one is already active in
PSpice.
If the old simulation has
completed, PSpice will load the
new simulation and run it.
-orIf the old simulation is running
or paused, PSpice will prompt
you to choose whether to run
the new simulation instead,
place it in the queue or cancel
it.
To extend a transient analysis
1
After you pause a transient analysis, click in the RunFor
text box on the PSpice toolbar.
2
Enter a new value for TSTOP.
3
Click on the Run toolbar button to resume the simulation.
The simulation will resume from the point at which it last
paused, and then run for the amount of time specified in
the RunFor text box, at which point it will pause again.
Note: Each time you resume the simulation after changing
TSTOP, the transient analysis will always pause when
completed. In this way, you can continue extending the
analysis indefinitely. If the simulation is paused before
TSTOP is reached, and you enter a value in the RunFor
402
PSpice User's Guide
Product Version 10.5
Setting up analyses
text box and click the Run toolbar button, PSpice will
run for the time specified and then pause. If you click
the Run button and if the total time has not yet reached
TSTOP, PSpice will run until TSTOP. If you pause the
simulation while it is in the middle of a RunFor
operation and then resume the simulation, PSpice will
complete the RunFor operation. If you click the Run
button while the simulation is paused in the middle of a
RunFor operation, PSpice will run until TSTOP is
reached.
PSpice User's Guide
403
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Interrupting a simulation
In PSpice, you have the ability to interrupt (pause) a
simulation, change certain runtime parameters, and then
resume the simulation from the point at which it was paused
using the new parameters.
Note: The new parameters are temporary values and are not
saved in the simulation profile. However, they are
logged in the output file so that you can refer to them
later.
When a simulation has been paused, you can change the
following runtime parameters in the Edit Runtime Settings
dialog box:
❑
RELTOL
❑
ABSTOL
❑
VNTOL
❑
GMIN
❑
TSTOP
❑
TMAX
❑
ITL1
❑
ITL2
❑
ITL4
Note: For more details about using these runtime
parameters, see the online PSpice Reference Guide.
The PSpice Runtime Settings dialog box will appear
automatically whenever a simulation fails to converge. (In
such cases, the simulation will be paused automatically.) It will
also appear if you attach PSpice to a simulation that was
paused in the background. (For more information about
managing background simulations, see Using the Simulation
Manager on page 409.)
404
PSpice User's Guide
Product Version 10.5
Setting up analyses
To interrupt a simulation and change parameters
1
In PSpice, from the Simulation menu, choose Edit
Runtime Settings.
The PSpice Runtime Settings dialog box appears.
2
If you want to use the original value for a particular
parameter, click the Use Original Value check box for that
parameter.
The original parameter values are derived from the
simulation profile. By default, the Use Original Value
check boxes are checked (enabled).
3
If you want to change one or more parameters, enter new
values for each of the runtime parameters you want to
change in the text boxes under the column Change To.
If a Change To text box is grayed out, uncheck the Use
Original Value check box.
4
Click OK & Resume Simulation to resume the simulation
with the new parameters.
Note: If you do not want to resume the simulation, but merely
want to exit this dialog box and preserve the values you
entered, click OK. If you run the simulation later, the
new parameters will be applied. If you want to exit this
dialog box without preserving the values, click Cancel.
PSpice User's Guide
405
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
Scheduling changes to runtime parameters
You may want to predefine a set of values for a parameter and
schedule these values to take effect at various time intervals
during a long simulation. For instance, you may want to use a
smaller time step value during periods where the input
stimulus changes rapidly, but otherwise use a larger value.
You can set up automatic changes to certain runtime
parameters that will occur at scheduled times during a
simulation. By scheduling the changes, you don't have to
interrupt the simulation manually, and can even run it in a
batch mode in the background.
The following runtime parameters can be changed at
scheduled times during a simulation. Note that these only
apply to transient analysis; you cannot interact with other
analysis types.
❑
RELTOL
❑
ABSTOL
❑
VNTOL
❑
GMIN
❑
ITL4
Note: For more details about using these runtime
parameters, see the online PSpice Reference Guide.
PSpice command syntax for scheduling parameter changes
You can schedule parameter changes by entering them either
in the Maximum Step Size text box in the Simulation Profile or
in a text file using the new expression SCHEDULE, and then
including that file in the simulation profile settings.
The expression SCHEDULE is a piecewise constant function
(from time x forward use y) and takes the form:
SCHEDULE(x1,y1,x2,y2…xn,yn)
406
PSpice User's Guide
Product Version 10.5
Setting up analyses
where x is the time value, which must be x >= 0, and
y is the value of the associated parameter. You must
include an entry for time = 0.
When used with the .OPTIONS command, the syntax is as
follows:
.OPTIONS <Parameter Name>=
{SCHEDULE(<time-value>, <parameter value>,
<time-value>, <parameter value>, …)}
For example,
.OPTIONS RELTOL={SCHEDULE( 0s,.001,2s,.005)}
indicates that RELTOL should have a value of 0.001 from time
0 up to time 2s, and a value of 0.005 from time 2s and beyond
(that is: RELTOL=.001 for t, where 0 <= t < 2s, and
RELTOL=.005 for t, where t >= 2s).
To schedule changes to runtime parameters
1
Open a standard text editor (such as Notepad) and create
a text file with the command syntax shown above, using
the appropriate values for the different parameters.
2
In Capture, open the design you want to simulate.
3
From the PSpice menu, choose Edit Simulation Profile.
The Simulation Settings dialog box appears.
PSpice User's Guide
4
Click on the Configuration Files tab
5
Click Include in the Category field to display the Include
files list.
6
Under the Filename text box, enter the name of the text
file you created in Step 1, or click the Browse button to
locate the file and enter the full path and filename.
7
Click the Add to Design button to include the file as part
of the circuit.
8
Click OK.
407
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
When you run the simulation, the scheduled parameter
changes will be included as part of the circuit file and the
simulation will run to completion automatically.
408
PSpice User's Guide
Product Version 10.5
Setting up analyses
Using the Simulation Manager
Overview of the Simulation Manager
PSpice includes a new Simulation Manager that provides
enhanced control over how multiple simulations are
processed. You can preempt the current simulation to run
another one first. Or, you can use the Simulation Manager to
monitor the progress of a set of batch simulations that were
set up and launched earlier.
Note: None of the earlier functionality of batch processing
has been lost. For more information, see Setting up
batch simulations on page 395.
The PSpice Simulation Manager provides a familiar,
easy-to-use interface for controlling how multiple simulations
are processed.
The Simulation Manager allows you to do the following:
PSpice User's Guide
■
add or delete simulations
■
start, stop or pause simulations
■
rearrange the order of the simulations in the queue
■
attach PSpice to a simulation to make it the active display
409
Chapter 8
Setting up analyses and starting simulation
■
Product Version 10.5
view the status and progress of simulations running in the
background
You can accomplish most of these functions by selecting the
desired simulation in the list, then clicking on the appropriate
toolbar button to execute the command.
Note: For simulations that are queued in the Simulation
Manager, the setting in the Simulation Profile to start
Probe automatically is ignored. When a queued
simulation runs to completion and finishes, it will not be
loaded into Probe. You must do this manually if you
want to see the results of that simulation.
Accessing the Simulation Manager
The Simulation Manager is invoked whenever you start a new
simulation, either from PSpice or from a front-end design entry
tool. Since it is active as long as a simulation is running in the
background, you can also call up the Simulation Manager from
the Windows system tray.
You can also launch the Simulation Manager by itself from the
Windows Start menu. You do not need to have PSpice running
in order to work with the Simulation Manager.
Understanding the information in the Simulation Manager
Every job listed in the Simulation Manager will have a specific
entry for Schedule, Status and Percent Complete. In addition,
certain color-coded icons are shown to the left of each
simulation file name to indicate their current state. A quick
glance over the list of jobs will tell you immediately where any
particular job is and how it will be processed. The following
410
PSpice User's Guide
Product Version 10.5
Setting up analyses
tables explain the meanings of the various categories and
states.
Icon
Explanation
The simulation is either in the queue and has not
been run yet, or has been run to completion.
The simulation is currently running.
The simulation has been paused and is on hold,
waiting to either be continued or stopped.
The simulation has been stopped and is not
completed.
Schedule
Explanation
queued
The simulation is in the queue. It will be run in
the order in which it is listed in the queue. (This
is the default setting.)
running
The simulation is currently running and
ongoing status information is displayed.
on hold
The simulation has been paused.
stopped
The simulation has been run completely, or
was stopped because of an error.
Note: You must manually restart a stopped
simulation if you want it to run again at a
later time.
PSpice User's Guide
Status
Explanation
not run
The simulation has not been started yet. (This
is the default setting.)
<status>
Basic status information about the progress of
the analysis will be displayed for a simulation
that is currently running.
411
Chapter 8
Setting up analyses and starting simulation
paused
Product Version 10.5
The simulation has been paused either
manually or automatically by the Simulation
Manager.
Note: If you change the default option that
automatically resumes paused
simulations in the queue, then you must
remember to manually resume a paused
simulation if you want it to continue at a
later time.
complete – The simulation has run to completion and no
no errors
errors were encountered.
errors
The simulation ran partially but stopped
automatically because errors were
encountered.
Percent
Explanation
<%>
The percentage of completion for a simulation.
This number increases as a simulation
progresses.
What the various versions of PSpice support
The following table identifies what functionality in the
Simulation Manager is available with each version of PSpice.
PSpice version
Functionality of Simulation Manager
PSpice Lite
Only one simulation may be running or
PSpice A/D Basics paused at a time.
The queue is run sequentially.
PSpice
PSpice A/D
One simulation may be running and
multiple simulations may be paused.
The queue is run sequentially.
412
PSpice User's Guide
Product Version 10.5
Setting up analyses
How the Simulation Manager handles errors during simulation
Since each simulation that runs in the background runs
independently, an error that occurs during one simulation will
not prevent the remaining jobs in the queue from running
subsequently, in order. The following common error conditions
may arise, but these will not prevent the Simulation Manager
from running the remaining simulations pending in the queue.
Simulation crash: If a simulation crashes for whatever reason,
the Simulation Manager will stop receiving progress updates.
After a certain period, the Simulation Manager will stop that
simulation and will automatically start the next job in the
queue.
Simulation pause: If a simulation pauses automatically and
requires manual intervention to continue, the Simulation
Manager will automatically start the next job in the queue.
Simulation stop: If a simulation stops automatically, the
Simulation Manager will automatically start the next job in the
queue.
Note: You must manually restart a stopped or paused
simulation if you want it to run again at a later time. You
will not be able to shut down the Simulation Manager
until all stopped and paused simulations have been
deleted.
Setting up multiple simulations
With the Simulation Manager, you can set up any number of
batch simulations to be run sequentially in the background
while you do other work in PSpice. Each new simulation that
you set up will be added to the bottom of the simulation queue
and will be assigned the schedule category "queued". It will be
run after all other queued jobs ahead of it have been run.
Once a job has been added, you can change its position in the
queue, start, stop or pause it, or make other modifications to
its status.
PSpice User's Guide
413
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
To add a simulation to the queue
1
From the File menu, choose Add Simulation or click the
Add Simulation button on the toolbar.
2
Locate the file (.SIM, .CIR) you wish to add to the queue.
Alternately, you can add a simulation to the queue by starting
the PSpice simulation directly from within the front-end tool
you are using, such as OrCAD Capture.
Note: If one simulation is already running in the Simulation
Manager and you start another one, you will be
prompted to direct the Simulation Manager in how to
proceed with the new simulation. For more information
about the different ways to handle this situation, see
Setting options in the Simulation Manager on
page 415.
Starting, stopping, and pausing simulations
In the Simulation Manager, you can easily manage the various
batch simulations in the queue. The most fundamental
controls that are provided are the ability to start a simulation,
stop it, or pause it temporarily.
To start a simulation from the Simulation Manager
1
Select a simulation in the list.
2
From the Simulation menu, choose Run or click the Run
Selected button on the toolbar.
To stop a simulation from the Simulation Manager
1
Select the simulation that is currently running.
2
From the Simulation menu, choose Stop or click the Stop
Selected button on the toolbar.
To pause a simulation from the Simulation Manager
1
414
Select the simulation that is currently running.
PSpice User's Guide
Product Version 10.5
Setting up analyses
2
From the Simulation menu, choose Pause or click the
Pause Selected button on the toolbar.
Attaching PSpice to a simulation
A simulation that is running in the Simulation Manager will not
be loaded into PSpice or displayed in Probe while it is running.
This allows you to work on a different design in the PSpice
application while a simulation is running in the Simulation
Manager.
Note: If you start a new simulation from within PSpice while
another is running in the queue in the Simulation
Manager, the Simulation Manager must decide how to
treat the new job. You will be prompted to choose
whether you want the new job to preempt the current
simulation and start running immediately. For more
details, click Setting options in the Simulation Manager
on page 415.
If you want to display a different simulation in PSpice by
choosing from the list of jobs in the Simulation Manager, you
can attach PSpice to a particular job in the queue.
To attach PSpice to a simulation
1
Select the simulation you want to attach PSpice to.
2
From the View menu, choose Simulation Results.
The PSpice program will activate and the results of the
simulation you selected will become the current display in
Probe. If the simulation is currently running, you will be able to
view the marching waveforms.
Setting options in the Simulation Manager
Each time you add a new simulation while another is running,
the Simulation Manager must decide how to treat the new job.
The default setting is to add the new simulation to the bottom
of the queue and continue running whatever job is currently
being simulated.
PSpice User's Guide
415
Chapter 8
Setting up analyses and starting simulation
Product Version 10.5
You can change this default so that the Simulation Manager
will start each new simulation immediately and either stop or
pause whatever job is currently running. The options you can
choose from are explained in the procedure below.
You can also choose to have the Options dialog box display
each time you add a new simulation, or not show this
anymore. If you disable the prompting, you can always enable
it again using the following procedure.
In addition, you can define how paused simulations should be
handled by the Simulation Manager. You can configure them
to be resumed automatically after the previous simulation
stops, or you can choose to leave them in a paused state until
you manually resume them.
To set the default options for the Simulation Manager
1
From the Tools menu, choose Options.
The Options dialog box appears.
416
PSpice User's Guide
Product Version 10.5
Setting up analyses
2
3
PSpice User's Guide
In the top frame dealing with simulations that are already
running, click the appropriate radio button for the option
you wish to set.
Radio button
Function
Display the
simulation in the
queue.
The simulation that is currently
running will be displayed in
PSpice. The new simulation will
be added to the bottom of the
queue and will be run after all
other jobs in the queue have
been run. (This is the default
setting.)
Pause the current
simulation and run
the new one.
The simulation that is currently
running will be paused. The
new simulation will be started
immediately. You must
remember to resume the
paused simulation later if you
want it to continue.
Stop the current
simulation and run
the new one.
The simulation that is currently
running will be stopped. The
new simulation will be started
immediately. You must
remember to restart the
stopped simulation later if you
want it to run again.
If you want the Options dialog box to appear as a
reminder each time you add a new simulation, be sure to
check the Always Prompt box. (The default setting is to
enable this feature.)
417
Chapter 8
Setting up analyses and starting simulation
4
Product Version 10.5
In the bottom frame dealing with paused simulations, click
the appropriate radio button for the option you wish to set.
Radio button
Function
Resume
simulating.
The first paused simulation in the
list will automatically resume after
the previous simulation has
stopped. (This is the default
setting.)
Wait for user
intervention.
The Simulation Manager will not
resume any paused simulations
automatically. You must intervene
manually to resume them.
Note: If you enable this radio
button, you must remember
to intervene manually if you
want paused simulations to
resume later.
5
418
Click OK to save the settings.
PSpice User's Guide
DC analyses
9
Chapter overview
This chapter describes how to set up DC analyses and
includes the following sections:
PSpice User's Guide
■
DC Sweep on page 420
■
Bias point on page 429
■
Small-signal DC transfer on page 431
■
DC sensitivity on page 434
419
Chapter 9
DC analyses
Product Version 10.5
DC Sweep
Minimum requirements to run a DC sweep analysis
Minimum circuit design requirements
Swept variable type
Requirement
voltage source
voltage source with a DC
specification (VDC, for example)
temperature
none
current source
current source with a DC
specification (IDC, for example)
model parameter
PSpice A/D model (.MODEL)
global parameter
global parameter defined with a
parameter block (.PARAM)
Minimum program setup requirements
1
420
In Capture, select New Simulation Profile or Edit
Simulation Profile from the PSpice menu. (If this is a new
simulation, enter the name of the profile and click OK.)
PSpice User's Guide
Product Version 10.5
Chapter overview
The Simulation Settings dialog box appears.
2
Under Analysis type, select DC Sweep.
3
For the Primary Sweep option, enter the necessary
parameter values and select the appropriate check boxes
to complete the analysis specifications.
4
Click OK to save the simulation profile.
5
Select Run under the PSpice menu to start the
simulation.
Note: Do not specify a DC sweep and a parametric analysis
for the same variable.
Overview of DC sweep
The DC sweep analysis causes a DC sweep to be performed
on the circuit. DC sweep allows you to sweep a source
(voltage or current), a global parameter, a model parameter, or
the temperature through a range of values. The bias point of
the circuit is calculated for each value of the sweep. This is
useful for finding the transfer function of an amplifier, the high
and low thresholds of a logic gate, and so on.
For the DC sweep analysis specified in Figure 9-1, the voltage
source V1 is swept from -0.125 volts to 0.125 volts by steps of
0.005. This means that the output has
(0.125 + 0.125)/0.005 +1 = 51 steps or simulation points.
A source with a DC specification (such as VDC or IDC) must
be used if the swept variable is to be a voltage type or current
source. To set the DC value, select Properties from the Edit
menu, then click on the cell under the DC column and type in
its value.
The default DC value of V1 is overridden during the DC sweep
analysis and is made to be the swept value. All of the other
sources retain their values.
After running the analysis, the simulation output file
(EXAMPLE.OUT for the EXAMPLE.OPJ circuit in Figure 9-1)
PSpice User's Guide
421
Chapter 9
DC analyses
Product Version 10.5
contains a table of voltages relating V1, node OUT1, and node
OUT2.
Figure 9-1 Example schematic EXAMPLE.OPJ.
Note: The example circuit EXAMPLE.OPJ is provided with
the program installation.
To calculate the DC response of an analog circuit, PSpice
removes time from the circuit. This is done by treating all
capacitors as open circuits, all inductors as shorts, and using
only the DC values of voltage and current sources. A similar
approach is used for digital devices: all propagation delays are
set to zero, and all stimulus generators are set to their
time-zero values.
In order to solve the circuit equations, PSpice uses an iterative
algorithm. For analog devices, the equations are continuous,
and for digital devices, the equations are Boolean. If PSpice
cannot get a self-consistent result after a certain number of
iterations, the analog/digital devices are forced to the X value,
and more iterations are done. Since X as input to a digital
component gives X as output, the Boolean equations can
always be solved this way.
If a digital node cannot be driven by known values during the
DC iterations (for instance, the output of a flip-flop with the
clock line held low), then its DC state will be X. Depending on
the circuit, some, none, or all of the digital nodes may have the
state X when the bias point is calculated.
422
PSpice User's Guide
Product Version 10.5
Chapter overview
Setting up a DC stimulus
To run a DC sweep or small-signal DC transfer analysis, you
need to place and connect one or more independent sources
and then set the DC voltage or current level for each source.
To set up a DC stimulus
1
Place and connect one of these symbols in your
schematic:
Table 9-1
For voltage input
Use
this...
When you are running...
VDC
A DC Sweep and/or Bias Point
(transfer function) analysis only.
VSRC
Multiple analysis types including DC
Sweep and/or Bias Point (transfer
function).
Table 9-2
For current input
PSpice User's Guide
Use
this...
When you are running...
IDC
A DC Sweep and/or Bias Point
(transfer function) analysis only.
ISRC
Multiple analysis types including DC
Sweep and/or Bias Point (transfer
function).
2
Double-click the symbol instance to display the Parts
spreadsheet appears.
3
Click in the cell under the DC column to edit its value.
423
Chapter 9
DC analyses
Product Version 10.5
4
Define the DC specification as follows:
Table 9-3
5
Set this
attribute...
To this value...
DC
DC_level
where DC_level is in volts or
amps (units are optional).
Click OK twice to exit the dialog boxes.
Note: If you are planning to run an AC or transient analysis in
addition to a DC analysis, see the following:
❑
Using time-based stimulus parts with AC and DC
properties on page 137 for other source symbols that
you can use.
❑
Using VSRC or ISRC parts on page 138 to find out
how to specify the TRAN attribute for a time-based
input signal when using VSRC or ISRC symbols.
Nested DC sweeps
A second sweep variable can be selected after a primary
sweep value has been specified in the DC Sweep dialog box.
When you specify a secondary sweep variable, it forms the
outer loop for the analysis. That is, for every increment of the
424
PSpice User's Guide
Product Version 10.5
Chapter overview
second sweep variable, the first sweep variable is stepped
through its entire range of values.
To set up a nested sweep
PSpice User's Guide
1
Under Options, select the Secondary Sweep box for the
DC Sweep Analysis type.
2
Enter the necessary parameter values and select the
appropriate check boxes to complete the analysis
specifications.
425
Chapter 9
DC analyses
Product Version 10.5
Curve families for DC sweeps
When a nested DC sweep is performed, the entire curve
family is displayed. That is, the nested DC sweep is treated as
a single data section (or you can think of it as a single PSpice
run).
Figure 9-2 Curve family example schematic
For the circuit shown in Figure 9-2, you can set up a DC sweep
analysis with an outer sweep of the voltage source VG and an
inner sweep of the voltage source VD as listed in Table 9-4.
Table 9-4 Curve family example setup
Primary
sweep
Secondary
sweep
Swept Var Type voltage source voltage source
426
Sweep Type
linear
linear
Name
VD
VG
Start Value
0
0
End Value
5
2
Increment
0.1
0.5
PSpice User's Guide
Product Version 10.5
Chapter overview
When the DC sweep analysis is run, add a current marker at
the drain pin of M1 and display the simulation results in
PSpice. The result will look like Figure 9-3.
Figure 9-3 Device curve family.
Note: In Capture, from the PSpice menu, point to Markers,
then choose Mark Current Into Pin to add a current
marker.
To add a load line for a resistor, add a trace that computes the
load line from the sweep voltage. Assume that the X axis
variable is the sweep voltage V_VD, which runs from 0 to 5
volts. The expression which will add a trace that is the load line
for a 50 kohm resistor is:
(5V-V_VD)/50K
Note: V_VD is the hierarchical name for VD created by
netlisting the schematic.
This can be useful for determining the bias point for each
member of a curve family as shown in Figure 9-4.
PSpice User's Guide
427
Chapter 9
DC analyses
Product Version 10.5
Figure 9-4 Operating point determination for
each member of the curve family.
428
PSpice User's Guide
Product Version 10.5
Chapter overview
Bias point
Minimum requirements to run a bias point analysis
Minimum circuit design requirements
None.
Minimum program setup requirements
1
Under Analysis type in the Simulation Settings dialog box,
select Bias Point.
2
For the General Settings option, enter the necessary
parameter values and select the appropriate check boxes
to complete the analysis specifications.
3
Click OK to save the simulation profile.
4
In Capture, from the PSpice menu, select Run to start the
simulation.
Overview of bias point
The bias point is calculated for any analysis whether or not the
Bias Point analysis is enabled in the Simulation Settings
dialog box. However, additional information is reported when
the Bias Point analysis is enabled. Also see Save and load bias
point on page 746.
When Bias Point analysis is not enabled, only analog node
voltages and digital node states are reported to the output file.
When the Bias Point analysis is enabled, the following
information is reported to the output file:
PSpice User's Guide
■
a list of all analog node voltages
■
a list of all digital node states
■
the currents of all voltage sources and their total power
■
a list of the small-signal parameters for all devices
429
Chapter 9
DC analyses
Product Version 10.5
If Bias Point is enabled, you can suppress the reporting of the
bias point analog and digital node values, as follows:
430
1
Under the Options tab in the Simulation Settings dialog
box, select Output file in the Category box.
2
Uncheck the box for Bias point node voltages (NOBIAS).
PSpice User's Guide
Product Version 10.5
Chapter overview
Small-signal DC transfer
Minimum requirements to run a small-signal DC transfer analysis
Minimum circuit design requirements
■
The circuit should contain an input source, such as
VSRC.
Minimum program setup requirements
PSpice User's Guide
1
Under Analysis type in the Simulation Settings dialog box,
select Bias Point.
2
Specify the name of the input source desired. See Output
variables on page 376 for a description of output variable
formats.
3
Click OK to save the simulation profile.
4
In Capture, from the PSpice menu, select Run to start the
simulation.
431
Chapter 9
DC analyses
Product Version 10.5
Overview of small-signal DC transfer
The small-signal DC transfer analysis calculates the
small-signal transfer function by transforming the circuit
around the bias point and treating it as a linear circuit. The
small-signal gain, input resistance, and output resistance are
calculated and reported.
The digital devices themselves are not included in the
small-signal analysis. A gate, for example, does not have a
frequency response. Instead, all the digital devices hold the
states that were calculated when solving for the bias point.
However, for N and O devices in the analog/digital interface
subcircuits, the analog side has a well-defined linear
equivalent.
To calculate the small-signal gain, input resistance, and
output resistance
1
In the Bias Point dialog box, select Calculate small-signal
DC gain (.TF).
2
Specify the value for either an output voltage or the
current through a voltage source in the To Output variable
box.
For example, entering V(a,b) as the output variable
specifies that the output variable is the output voltage
432
PSpice User's Guide
Product Version 10.5
Chapter overview
between two nets, a and b. Entering I(VDRIV) as the
output variable specifies that the output variable is the
current through a voltage source VDRIV.
3
Specify the input source name in the Calculate
small-signal DC gain (.TF) portion of the Bias Point dialog
box.
The gain from the input source to the output variable is
calculated along with the input and output resistances.
For example, if you enter V(OUT2)as the output variable
and V1 as the input source, the input resistance for V1 is
calculated, the output resistance for V(OUT2) is
calculated, and the gain from V1 to V(OUT2) is
calculated. All calculations are reported to the simulation
output file.
PSpice User's Guide
433
Chapter 9
DC analyses
Product Version 10.5
DC sensitivity
Minimum requirements to run a DC sensitivity analysis
Minimum circuit design requirements
None.
Minimum program setup requirements
434
1
In the Bias Point dialog box, select Perform Sensitivity
analysis (.SENS).
2
Enter the required value(s) in the Output variable(s) box.
3
Click OK to save the simulation profile. (Be sure you give
the new profile an appropriate name under the General
tab prior to saving.)
4
In Capture, from the PSpice menu, select Run to start the
simulation.
PSpice User's Guide
Product Version 10.5
Chapter overview
Overview of DC sensitivity
DC sensitivity analysis calculates and reports the sensitivity of
one node voltage to each device parameter for the following
device types:
■
resistors
■
independent voltage and current sources
■
voltage and current-controlled switches
■
diodes
■
bipolar transistors
The sensitivity is calculated by linearizing all devices around
the bias point. Purely digital devices hold the states calculated
when solving for the bias point as discussed in Small-signal
DC transfer on page 431.
PSpice User's Guide
435
Chapter 9
436
DC analyses
Product Version 10.5
PSpice User's Guide
AC analyses
10
Chapter overview
This chapter describes how to set up AC sweep and noise
analyses.
PSpice User's Guide
■
AC sweep analysis on page 438 describes how to set up
an analysis to calculate the frequency response of your
circuit. This section also discusses how to define an AC
stimulus and how PSpice treats nonlinear devices in an
AC sweep.
■
Noise analysis on page 448 describes how to set up an
analysis to calculate device noise contributions and total
input and output noise.
437
Chapter 10
AC analyses
Product Version 10.5
AC sweep analysis
Setting up and running an AC sweep
The following procedure describes the minimum setup
requirements for running an AC sweep analysis. For more
detail on any step, go to the pages referenced in the sidebars.
To set up and run an AC sweep
1
Place and connect a voltage or current source with an AC
input signal.
To find out how, see Setting up an AC stimulus on
page 439.
2
From the PSpice menu, select New Simulation Profile or
Edit Simulation Profile. (If this is a new simulation, enter
the name of the profile and click OK.)
The Simulation Settings dialog box appears.
3
Choose AC Sweep/Noise in the Analysis type list box.
4
Specify the required parameters for the AC sweep or
noise analysis you want to run.
To find out how, see Setting up an AC analysis on
page 442.
5
Click OK to save the simulation profile.
6
From the PSpice menu, select Run to start the simulation.
What is AC sweep?
AC sweep is a frequency response analysis. PSpice
calculates the small-signal response of the circuit to a
combination of inputs by transforming it around the bias point
and treating it as a linear circuit. Here are a few things to note:
■
438
Nonlinear devices, such as voltage- or current-controlled
switches, are transformed to linear circuits about their
bias point value before PSpice A/D runs the linear
PSpice User's Guide
Product Version 10.5
Chapter overview
(small-signal) analysis. To find out more, see How PSpice
treats nonlinear devices on page 446.
■
Digital devices hold the states that PSpice calculated
when solving for the bias point.
■
Because AC sweep analysis is a linear analysis, it only
considers the gain and phase response of the circuit; it
does not limit voltages or currents.
The best way to use AC sweep analysis is to set the source
magnitude to one. This way, the measured output equals the
gain, relative to the input source, at that output.
Setting up an AC stimulus
To run an AC sweep analysis, you need to place and connect
one or more independent sources and then set the AC
magnitude and phase for each source.
Note: Unlike DC sweep, the AC Sweep/Noise dialog box
does not include an input source option. Instead, each
independent source in your circuit contains its own AC
specification for magnitude and phase.
PSpice User's Guide
439
Chapter 10
AC analyses
Product Version 10.5
To set up an AC stimulus
1
Place and connect one of these symbols in your
schematic:
Table 10-1
For voltage input
Use
this...
When you are running...
VAC
An AC sweep analysis only.
VSRC
Multiple analysis types including AC
sweep.
Table 10-2
For current input
Use
this...
When you are running...
IAC
An AC sweep analysis only.
ISRC
Multiple analysis types including AC
sweep.
If you are planning to run a DC or transient analysis in
addition to an AC analysis, see If you want to specify
multiple stimulus types on page 137 for additional
information and source symbols that you can use.
2
440
Double-click the symbol instance to display the Parts
spreadsheet.
PSpice User's Guide
Product Version 10.5
Chapter overview
3
Click in the cell under the appropriate property column to
edit its value. Depending on the source symbol that you
placed, define the AC specification as follows:
Table 10-3
For VAC or IAC
Set this
property...
To this value...
ACMAG
AC magnitude in volts (for VAC) or
amps (for IAC); units are optional.
ACPHASE
Optional AC phase in degrees.
Table 10-4
For VSRC or
ISRC
Set this
property...
To this value...
AC
Magnitude_value [phase_value]
where magnitude_value is in volts or
amps (units are optional) and the
optional phase_value is in degrees.
If you are also planning to run a transient analysis, see
Using VSRC or ISRC parts on page 138 to find out how
to specify the TRAN property.
PSpice User's Guide
441
Chapter 10
AC analyses
Product Version 10.5
Setting up an AC analysis
To set up the AC analysis
1
From the PSpice menu, choose New Simulation Profile or
Edit Simulation Settings. (If this is a new simulation, enter
the name of the profile and click OK.)
The Simulation Settings dialog box appears.
2
Choose AC Sweep/Noise in the Analysis type list box.
3
Under Options, select General Settings if it is not already
enabled.
4
Set the number of sweep points as follows:
Table 10-5
To sweep frequency... Do this...
linearly
442
Under AC Sweep Type, click
Linear, and enter the total
number of points in the sweep
in the Total Points box.
PSpice User's Guide
Product Version 10.5
Chapter overview
Table 10-5
To sweep frequency... Do this...
logarithmically by
decades
Under AC Sweep Type, click
Logarithmic, select Decade
(default), and enter the total
number of points per decade
in the Total Points box.
logarithmically by
octaves
Under AC Sweep Type, click
Logarithmic, select Octave,
and enter the total number of
points per octave in the Total
Points box.
5
In the Start Frequency and End Frequency text boxes,
enter the starting and ending frequencies, respectively,
for the sweep.
6
Click OK to save the simulation profile.
Note: If you also want to run a noise analysis, then before
clicking OK, complete the Noise Analysis frame in this
dialog box as described in Setting up a noise analysis
on page 450.
PSpice User's Guide
443
Chapter 10
AC analyses
Product Version 10.5
AC sweep setup in example.opj
If you look at the example circuit, EXAMPLE.OPJ, provided
with your installed programs, you’ll find that its AC analysis is
set up as shown in Figure 10-2.
Figure 10-1 Circuit diagram for EXAMPLE.OPJ.
Note: The source, V1, is a VSIN source that is normally used
for setting up sine wave signals for a transient analysis.
It also has an AC property so that you can use it for an
AC analysis.
To find out more about VSIN and other source symbols
444
PSpice User's Guide
Product Version 10.5
Chapter overview
that you can use for AC analysis, see Using time-based
stimulus parts with AC and DC properties on page 137.
Figure 10-2 AC analysis setup for EXAMPLE.OPJ.
Frequency is swept from 100 kHz to 10 GHz by decades, with
10 points per decade. The V1 independent voltage source is
the only input to an amplifier, so it is the only AC stimulus to
this circuit. Magnitude equals 1 V and relative phase is left at
zero degrees (the default). All other voltage sources have zero
AC value.
PSpice User's Guide
445
Chapter 10
AC analyses
Product Version 10.5
How PSpice treats nonlinear devices
An AC Sweep analysis is a linear or small-signal analysis. This
means that nonlinear devices must be linearized to run the
analysis.
What’s required to transform a device into a linear circuit
In order to transform a device (such as a transistor amplifier)
into a linear circuit, you must do the following:
1
Compute the DC bias point for the circuit.
2
Compute the complex impedance and/or
transconductance values for each device at this bias
point.
3
Perform the linear circuit analysis at the frequencies of
interest by using simplifying approximations.
Example: Replace a bipolar transistor in common-emitter
mode with a constant transconductance (collector current
proportional to base-emitter voltage) and a number of
constant impedances.
What PSpice does
PSpice automates this process for you. PSpice computes the
partial derivatives for nonlinear devices at the bias point and
uses these to perform small-signal analysis.
Example: nonlinear behavioral modeling block
Suppose you have an analog behavioral modeling block that
multiplies V(1) by V(2). Multiplication is a nonlinear operation.
To run an AC sweep analysis on this block, the block needs to
be replaced with its linear equivalent. To determine the linear
equivalent block, PSpice needs a known bias point.
446
PSpice User's Guide
Product Version 10.5
Chapter overview
Using a DC source
Consider the circuit shown below.
At the DC bias point, PSpice calculates the partial derivatives
which determine the linear response of the multiplier as
follows:
∂V ( Out ) ∂V ( Out )
V ( Out ) = ---------------------- + ---------------------∂V ( In1 ) ∂V ( In2 )
˙ ) + 2. 0
= 2.V ( In1
For this circuit, this equation reduces to:
V ( Out ) = 2V ( In1 )
This means that the multiplier acts as an amplifier of the AC
input with a gain that is set by the DC input.
Caution: multiplying AC sources
Suppose that you replace the 2 volt DC source in this example
with an AC source with amplitude 1 and no DC value (DC=0).
When PSpice computes the bias point, there are no DC
sources in the circuit, so all nodes are at 0 volts at the bias
point. The linear equivalent of the multiplier block is a block
with gain 0, which means that there is no output voltage at the
fundamental frequency. This is exactly how a double-balanced
mixer behaves. In practice, this is a simple multiplier.
Note: A double-balanced mixer with inputs at the same
frequency would produce outputs at DC at twice the
input frequency, but these terms cannot be seen with a
linear, small-signal analysis.
PSpice User's Guide
447
Chapter 10
AC analyses
Product Version 10.5
Noise analysis
Setting up and running a noise analysis
The following procedure describes the minimum setup
requirements for running a noise analysis. For more detail on
any step, go to the pages referenced in the sidebars.
To set up and run an AC sweep
1
Place and connect a voltage or current source with an AC
input signal.
To find out how, see Setting up an AC stimulus on
page 439.
2
Set up the AC sweep simulation specifications.
To find out how, see Setting up an AC analysis on page 442.
3
Set up the noise simulation specifications and enable the
analysis in the AC Sweep/Noise portion of the Simulation
Settings dialog box.
To find out how, see Setting up a noise analysis on
page 450.
448
4
Click OK to save the simulation profile.
5
From the PSpice menu, choose Run to start the
simulation.
PSpice User's Guide
Product Version 10.5
Chapter overview
What is noise analysis?
When running a noise analysis, PSpice calculates and reports
the following for each frequency specified for the AC
Sweep/Noise analysis:
■
Device noise, which is the noise contribution propagated
to the specified output net from every resistor and
semiconductor device in the circuit; for semiconductor
devices, the device noise is also broken down into
constituent noise contributions where applicable
Example: Diodes have separate noise contributions from
thermal, shot, and flicker noise.
■
Total output and equivalent input noise
Table 10-6
This value... Means this...
Output noise
RMS sum of all the device contributions
propagated to a specified output net
Input noise
equivalent noise that would be needed
at the input source to generate the
calculated output noise in an ideal
(noiseless) circuit
How PSpice calculates total output and input noise
To calculate total noise at an output net, PSpice computes the
RMS sum of the noise propagated to the net by all
noise-generating devices in the circuit.
To calculate the equivalent input noise, PSpice then divides
total output noise by the gain from the input source to the
output net. This results in the amount of noise which, if
injected at the input source into a noiseless circuit, would
produce the total noise originally calculated for the output net.
PSpice User's Guide
449
Chapter 10
AC analyses
Product Version 10.5
Setting up a noise analysis
To set up the noise analysis
1
From the PSpice menu, choose New Simulation Profile or
Edit Simulation Profile. (If this is a new simulation, enter
the name of the profile and click OK.)
The Simulation Settings dialog box appears.
450
2
Choose AC Sweep/Noise in the Analysis type list box.
3
Under Options, select General Settings if it is not already
enabled.
4
Specify the AC sweep analysis parameters as described
in Setting up an AC analysis on page 442.
5
Enable the Noise Analysis check box.
PSpice User's Guide
Product Version 10.5
Chapter overview
6
Enter the noise analysis parameters as follows:
Table 10-7
In this text
box...
Type this...
Output Voltage A voltage output variable of the form
V(node, [node]) where you want the
total output noise calculated.
To find out more about valid syntax,
see Output variables on page 376.
I/V Source
The name of an independent current or
voltage source where you want the
equivalent input noise calculated.
Note: If the source is in a lower level of
a hierarchical schematic,
separate the names of the
hierarchical devices with periods
(.).
Example: U1.V2
Interval
An integer n designating that at every
n th frequency, you want to see a table
printed in the PSpice output file (.OUT)
showing the individual contributions of
all of the circuit’s noise generators to
the total noise.
Note: In the Probe window, you can
view the device noise
contributions at every frequency
specified in the AC sweep. The
Interval parameter has no effect
on what PSpice writes to the
Probe data file.
7
PSpice User's Guide
Click OK to save the simulation profile.
451
Chapter 10
AC analyses
Product Version 10.5
Analyzing Noise in the Probe window
You can use these output variable formats to view traces for
device noise contributions and total input or output noise at
every frequency in the analysis.
For a break down of noise output variables by supported
device type, see Table 17-17 on page 698.
To view this...
Use this output
variable...
Which is represented by this
equation1...
Flicker noise for a device
NFID(device_name)
NFIB(device_name)
noise ∝
Shot noise for a device
NSID(device_name)
NSIB(device_name)
NSIC(device_name)
For diodes and BJTs:
noise ∝
af
I
k f ⋅ ----bf
2qI
For GaAsFETs, JFETs, and
MOSFETs:
noise ∝
dI 2
4kT ⋅ ------- ⋅ --dV 3
noise ∝
4kT
---------R
Thermal noise generated by NRLO(device_name)
equivalent resistances in the NRHI(device_name)
output of a digital device
noise ∝
4kT
---------R
Total noise for a device
NTOT(device_name)
Sum of all contributors in
device_name
Total output noise for the
circuit
NTOT(ONOISE)
RMS-summed output noise
for the circuit
V(ONOISE)
Thermal noise for the RB,
RC, RD, RE, RG, or RS
constituent of a device,
respectively
NRB(device_name)
NRC(device_name)
NRD(device_name)
NRE(device_name)
NRG(device_name)
NRS(device_name)
Equivalent input noise for the V(INOISE)
circuit
452
∑
NTOT ( device )
device
RMS sum of all contributors
( NTOT ( ONOISE ) )
V ( ONOISE )
--------------------------------gain
PSpice User's Guide
Product Version 10.5
Chapter overview
1. To find out more about the equations that describe noise behavior, refer to the appropriate device
type in the Analog Devices chapter in the online PSpice Reference Guide .
About noise units
Table 10-8
This type of noise output variable...
Is reported in
these units...
2
Device contribution of the form Nxxx
( volts ) ⁄ ( Hz )
Total input or output noise of the form
V(ONOISE) or V(INOISE)
( volts ) ⁄ ( Hz )
Example
You can run a noise analysis on the circuit shown in
Figure 10-1 on page 444.
To run a noise analysis on the example:
In Capture, open the EXAMPLE.OPJ circuit provided in the
\tools\pspice\capture_samples\anasim\example subdirectory.
1
From the PSpice menu, choose New Simulation Profile or
Edit Simulation Profile. (If this is a new simulation, enter
the name of the profile and click OK.)
The Simulation Settings dialog box appears.
PSpice User's Guide
2
Choose AC Sweep/Noise in the Analysis type list box.
3
Under Options, select General Settings if it is not already
enabled.
4
Enable the Noise Analysis check box.
5
Enter the following parameters for the noise analysis:
Output Voltage
V(OUT2)
I/V Source
V1
453
Chapter 10
AC analyses
Product Version 10.5
Interval
30
For a description of the
Interval parameter, see
Interval on page 451.
These settings mean that PSpice will calculate noise
contributions and total output noise at net OUT2 and
equivalent input noise from V1.
Figure 10-3 shows Probe traces for Q1’s constituent noise
sources as well as total noise for the circuit after simulating.
Notice that the trace for RMSSUM (at the top of the plot),
which is a macro for the trace expression
SQRT(NTOT(Q1) + NTOT(Q2) + NTOT(Q3) + ... ),
exactly matches the total output noise, V(ONOISE),
calculated by PSpice A/D.
454
PSpice User's Guide
Product Version 10.5
Chapter overview
To find out more about PSpice macros, refer to the online
PSpice Help.
Figure 10-3 Device and total noise traces for
EXAMPLE.OPJ.
Note: The source, V1, is a VSIN source that is normally used
for setting up sine wave signals for a transient analysis.
It also has an AC property so that you can use it for an
AC analysis.
To find out more about VSIN and other source symbols
that you can use for AC analysis, see Using time-based
stimulus parts with AC and DC properties on page 137.
Frequency is swept from 100 kHz to 10 GHz by decades, with
10 points per decade. The V1 independent voltage source is
PSpice User's Guide
455
Chapter 10
AC analyses
Product Version 10.5
the only input to an amplifier, so it is the only AC stimulus to
this circuit. Magnitude equals 1 V and relative phase is left at
zero degrees (the default). All other voltage sources have zero
AC value.
456
PSpice User's Guide
Parametric and temperature
analysis
11
Chapter overview
This chapter describes how to set up parametric and
temperature analyses. Parametric and temperature are both
simple multi-run analysis types.
This chapter includes the following sections:
PSpice User's Guide
■
Parametric analysis on page 458
■
Temperature analysis on page 467
457
Chapter 11
Parametric and temperature analysis
Product Version 10.5
Parametric analysis
Minimum requirements to run a parametric analysis
Note: Parametric analysis is not included in PSpice A/D
Basics.
Minimum circuit design requirements
■
Set up the circuit according to the swept variable type as
listed in Table 11-1.
■
Set up a DC sweep, AC sweep, or transient analysis.
Table 11-1 Parametric analysis circuit design
requirements
Swept variable type
Requirement
voltage source
voltage source with a DC
specification (VDC, for example)
temperature
none
current source
current source with a DC
specification (IDC, for example)
model parameter
PSpice A/D model
global parameter
global parameter defined with a
parameter block (PARAM)
Minimum program setup requirements
1
In the Simulation Settings dialog box, from the Analysis
type list box, select Time Domain (Transient).
See Setting up analyses on page 373 for a description of
the Simulation Settings dialog box.
2
458
Under Options, select Parametric Sweep if it is not
already enabled.
PSpice User's Guide
Product Version 10.5
Chapter overview
3
Specify the required parameters for the sweep.
4
Click OK to save the simulation profile.
5
From the PSpice menu, choose Run to start the
simulation.
Note: Do not specify a DC sweep and a parametric analysis
for the same variable.
Overview of parametric analysis
Parametric analysis performs multiple iterations of a specified
standard analysis while varying a global parameter, model
parameter, component value, or operational temperature. The
effect is the same as running the circuit several times, once for
each value of the swept variable.
See Parametric analysis on page 93 for a description of how
to set up a parametric analysis.
RLC filter example
This example shows how to perform a parametric sweep and
analyze the results with performance analysis.
PSpice User's Guide
459
Chapter 11
Parametric and temperature analysis
Product Version 10.5
Use performance analysis to derive values from a series of
simulator runs and plot these values versus a parameter that
varies between the simulator runs.
For this example, the derived values are the overshoot and the
rise time versus the damping resistance of the filter.
Entering the design
The schematic representation for the RLC filter
(RLCFILT.OPJ) is shown in Figure 11-1.
Figure 11-1 Passive filter schematic.
This series of PSpice runs varies the value of resistor R1 from
0.5 to 1.5 ohms in 0.1 ohm steps. Since the time-constant of
the circuit is about one second, perform a transient analysis of
approximately 20 seconds.
Create the circuit in Capture by placing a piecewise linear
independent current source (IPWL from SOURCE.OLB). Set
the current source properties as follows:
AC
T1
I1
T2
I2
T3
I3
=
=
=
=
=
=
=
1a
0s
0a
10ms
0a
10.1ms
1a
Place an instance of a resistor and set its VALUE property to
the expression, {R}. To define R as a global parameter, place
a PARAM pseudocomponent and use the Property Editor to
460
PSpice User's Guide
Product Version 10.5
Chapter overview
create a new property R and set its value to 0.5. Place an
inductor and set its value to 1H, place a capacitor and set its
value to 1, and place an analog ground symbol (0 from the
SOURCE.OLB library). Wire the schematic symbols together
as shown in Figure 11-1.
Running the simulation
Run PSpice A/D with the following analyses enabled:
transient
print step:
final time:
100ms
20s
parametric
swept var. type:
sweep type:
name:
start value:
end value:
increment:
global parameter
linear
R
0.5
1.5
0.1
After setting up the analyses, start the simulation by choosing
Run from the PSpice menu.
Using performance analysis to plot overshoot and rise time
After performing the simulation that creates the data file
RLCFILT.DAT, you can calculate the specified performance
analysis measurements.
When the simulation is finished, a list appears containing all of
the sections (runs) in the data file produced by PSpice. To use
the data from every run, select All and click OK in the Available
Selections dialog box. In the case of Figure 11-2, the trace
I(L1) from the ninth section was added by specifying the
following in the Add Traces dialog box:
-I(L1)@9
PSpice User's Guide
461
Chapter 11
Parametric and temperature analysis
Product Version 10.5
Note: To display the Add Traces dialog box, from the Trace
menu, choose Add Trace or click the Add Trace toolbar
button
.
Figure 11-2 Current of L1 when R1 is 1.5 ohms.
To run performance analysis
1
From the Trace menu, choose Performance Analysis.
2
Click OK.
PSpice resets the X-axis variable for the graph to be the
parameter that changed between PSpice runs. In the
example, this is the R parameter.
To see the rise time for the current through the inductor L1,
click the Add Trace toolbar button
and then enter:
genrise(-I(L1) )
Note: The genrise and overshoot measurements are
contained in the PSPICE.PRB file in the <target
installation directory>\PSpice\Common directory. For
legacy users, there are now two files in the
PSpice\Common directory:
462
❑
PSPICE_OLB.PRB uses goal function names
❑
PSPICE.PRB uses measurement names
PSpice User's Guide
Product Version 10.5
Chapter overview
Figure 11-3, shows how the rise time decreases as the
damping resistance increases for the filter.
Another Y axis can be added to the plot for the overshoot of
the current through L1 by selecting Add Y Axis from the Plot
menu. The Y axis is immediately added. Now click the Add
Trace toolbar button and enter:
overshoot(-I(L1) )
Figure 11-3 shows how the overshoot increases with
increasing resistance.
Figure 11-3 Rise time and overshoot vs. damping
resistance.
Troubleshooting tip
More than one PSpice run or data section is required for
performance analysis. Because one data value is derived for
each waveform in a related set of waveforms, at least two data
points are required to produce a trace.
Use Eval Goal Function (from the Trace menu) to evaluate a
goal function on a single waveform and produce a single data
point result.
PSpice User's Guide
463
Chapter 11
Parametric and temperature analysis
Product Version 10.5
Example: frequency response vs. arbitrary parameter
You can view a plot of the linear response of a circuit at a
specific frequency as one of the circuit parameters varies
(such as the output of a band pass filter at its center frequency
vs. an inductor value).
In this example, the value of a nonlinear capacitance is
measured using a 10 kHz AC signal and plotted versus its bias
voltage. The capacitance is in parallel with a resistor, so a
trace expression is used to calculate the capacitance from the
complex admittance of the R-C pair.
Note: This technique for measuring branch capacitances
works well in both simple and complex circuits.
Setting up the circuit
Enter the circuit in Capture as shown in Figure 11-4.
Figure 11-4 RLC filter
example circuit.
To create the capacitor model in the schematic editor:
1
Place a CBREAK part.
2
Select it so that it is highlighted.
3
From the Edit menu, choose PSpice Model.
4
In the Model Text frame, enter the following:
.model Cnln CAP(C=1 VC1=-0.01 VC2=0.05)
5
From the File menu, choose Save.
Set up the circuit for a parametric AC analysis (sweep Vbias),
and run PSpice. Include only the frequency of interest in the
AC sweep.
464
PSpice User's Guide
Product Version 10.5
Chapter overview
To display the results
Use PSpice to display the capacitance calculated at the
frequency of interest versus the stepped parameter.
1
Simulate the circuit.
2
Load all AC analysis sections.
3
From the Trace menu, choose Add Trace or click the Add
Trace toolbar button
.
4
Add the following trace expression:
IMG(-I(Vin)/V(1,0))/(2*3.1416*Frequency)
Or add the expression:
CvF(-I(Vin)/V(1,0))
Where CvF is a macro which measures the effective
capacitance in a complex conductance. Macros are defined
using the Macros command on the Trace menu. The CvF
macro should be defined as:
CvF(G)= IMG(G)/(2*3.1416*Frequency)
Note: -I(Vin)/V(1) is the complex admittance of the R-C
branch; the minus sign is required for correct polarity.
To use performance analysis to plot capacitance vs. bias
voltage
1
From the Trace menu, choose Performance Analysis.
2
Click Wizard.
3
Click Next>.
4
Click YatX in the Choose a Goal Function list, and then
click Next>.
5
In the Name of Trace text box, type the following:
CvF(-I(Vin)/V(1))
6
In the X value to get Y value at text box, type 10K.
7
Click Next>.
The wizard displays the gain trace for the first run to text
the goal function (YatX).
PSpice User's Guide
465
Chapter 11
Parametric and temperature analysis
8
Product Version 10.5
Click Finish.
The resultant plot is shown in Figure 11-5.
Figure 11-5 Plot of capacitance versus bias voltage.
466
PSpice User's Guide
Product Version 10.5
Chapter overview
Temperature analysis
Minimum requirements to run a temperature analysis
Minimum circuit design requirements
None.
Minimum program setup requirements
1
In the Simulation Settings dialog box, from the Analysis
type list box, select Time Domain (Transient).
See Setting up analyses on page 373 for a description of
the Simulation Settings dialog box.
PSpice User's Guide
2
Under Options, select Temperature Sweep if it is not
already enabled.
3
Specify the required parameters for the sweep.
4
Click OK to save the simulation profile.
5
From the PSpice menu, choose Run to start the
simulation.
467
Chapter 11
Parametric and temperature analysis
Product Version 10.5
Overview of temperature analysis
For a temperature analysis, PSpice reruns standard analyses
set in the Simulation Settings dialog box at different
temperatures.
Note: Running multiple analyses for different temperatures
can also be achieved using parametric analysis (see
Parametric analysis on page 458). With parametric
analysis, the temperatures can be specified either by
list, or by range and increments within the range.
You can specify zero or more temperatures. If no temperature
is specified, the circuit is run at 27˚C. If more than one
temperature is listed, the simulation runs once for each
temperature in the list.
Setting the temperature to a value other than the default
results in recalculating the values of temperature-dependent
devices. In EXAMPLE.OPJ (see Figure 11-6), the temperature
for all of the analyses is set to 35˚C. The values for resistors
RC1 and RC2 are recomputed based upon the CRES model
which has parameters TC1 and TC2 reflecting linear and
quadratic temperature dependencies.
Likewise, the Q3 and Q4 device values are recomputed using
the Q2N2222 model which also has temperature-dependent
parameters. In the simulation output file, these recomputed
device values are reported in the section labeled
TEMPERATURE ADJUSTED VALUES.
468
PSpice User's Guide
Product Version 10.5
Chapter overview
Figure 11-6 Example schematic EXAMPLE.OPJ.
Note: The example circuit EXAMPLE.OPJ is provided with
the installed programs.
PSpice User's Guide
469
Chapter 11
470
Parametric and temperature analysis
Product Version 10.5
PSpice User's Guide
Transient analysis
12
Chapter overview
This chapter describes how to set up a transient analysis and
includes the following sections:
PSpice User's Guide
■
Overview of transient analysis on page 472
■
Defining a time-based stimulus on page 474
■
The Stimulus Editor utility on page 476
■
Transient (time) response on page 487
■
Internal time steps in transient analyses on page 490
■
Switching circuits in transient analyses on page 491
■
Plotting hysteresis curves on page 492
■
Fourier components on page 493
471
Chapter 12
Transient analysis
Product Version 10.5
Overview of transient analysis
Minimum requirements to run a transient analysis
Minimum circuit design requirements
Circuit should contain one of the following:
■
An independent source with a transient specification (see
Table 12-1)
■
An initial condition on a reactive element
■
A controlled source that is a function of time
Minimum program setup requirements
1
From Capture’s PSpice menu, choose New Simulation
Profile or Edit Simulation Profile. (If this is a new
simulation, enter the name of the profile and click OK.)
The Simulation Settings dialog box appears.
2
Click the Analysis tab.
See Setting up analyses on page 373 for a description of
the Analysis Setup dialog box.
472
PSpice User's Guide
Product Version 10.5
PSpice User's Guide
Chapter overview
3
From the Analysis type list box, select Time Domain
(Transient).
4
Specify the required parameters for the transient analysis
you want to run.
5
Click OK to save the simulation profile.
6
From the PSpice menu, choose Run to start the
simulation.
473
Chapter 12
Transient analysis
Product Version 10.5
Defining a time-based stimulus
Overview of stimulus generation
Symbols that generate input signals for your circuit can be
divided into two categories:
■
those whose transient behavior is characterized
graphically using the Stimulus Editor
■
those whose transient behavior is characterized by
manually defining their properties within Capture
Note: Stimulus Editor is not included with PSpice A/D Basics
These symbols are summarized in Table 12-1.
Table 12-1 Stimulus symbols for time-based input
signals
Specified
by...
Symbol name
Description
Using the
Stimulus
Editor
VSTIM
voltage source
ISTIM
current source
DIGSTIM1
digital stimuli
DIGSTIM2
DIGSTIM4
DIGSTIM8
DIGSTIM16
DIGSTIM32
474
Note: Digital
stimuli are
not
supported
in PSpice.
PSpice User's Guide
Product Version 10.5
Chapter overview
Table 12-1 Stimulus symbols for time-based input
signals, continued
Specified
by...
Symbol name
Description
Defining
symbol
attribute
VSRC
voltage sources
VEXP
VPULSE
VPWL
VPWL_RE_FOREVER
VPWL_F_RE_FOREVER
VPWL_N_TIMES
VPWL_F_N_TIMES
VSFFM
VSIN
ISRC
IEXP
IPULSE
IPWL
IPWL_RE_FOREVER
IPWL_F_RE_FOREVER
IPWL_N_TIMES
IPWL_F_N_TIMES
ISFFM
ISIN
current sources
DIGCLOCK
digital clock signal
STIM1
STIM4
STIM8
STIM16
digital stimuli
FILESTIM1
digital file stimuli
FILESTIM2
Note: Digital
stimuli are
not
supported
in PSpice.
FILESTIM4
FILESTIM8
FILESTIM16
FILESTIM32
To use any of these source types, you must place the symbol
in your schematic and then define its transient behavior.
PSpice User's Guide
475
Chapter 12
Transient analysis
Product Version 10.5
Each property-characterized stimulus has a distinct set of
attributes depending upon the kind of transient behavior it
represents. For VPWL_F_xxx, IPWL_F_xxx, and FSTIM, a
separate file contains the stimulus specification. For
information on digital stimuli characterized by property, see
Chapter 14, “Digital simulation.”
As an alternative, the Stimulus Editor automates the process
of defining the transient behavior of stimulus devices. The
Stimulus Editor allows you to create analog stimuli which
generate sine wave, repeating pulse, exponential pulse,
single-frequency FM, and piecewise linear waveforms. It also
facilitates creating digital stimuli with complex timing relations.
This applies to both stimulus symbols placed in your
schematic as well as new ones that you might create.
The stimulus specification created using the Stimulus Editor is
saved to a file, automatically configured into the schematic,
and associated with the corresponding VSTIM, ISTIM, or
DIGSTIM part instance or symbol definition.
The Stimulus Editor utility
The Stimulus Editor is a utility that allows you to quickly set up
and verify the input waveforms for a transient analysis. You
can create and edit voltage sources, current sources, and
digital stimuli for your circuit. Menu prompts guide you to
provide the necessary parameters, such as the rise time, fall
time, and period of an analog repeating pulse, or the complex
timing relations with repeating segments of a digital stimulus.
Graphical feedback allows you to quickly verify the waveform.
See the Stimulus Editor online help for more information about
this utility.
Note: Stimulus Editor is not included with PSpice A/D Basics
Note: If you are using a PSpice product that does not include
the Stimulus Editor, you must use the
characterized-by-property sources listed in Table 12-1
on page 474.
476
PSpice User's Guide
Product Version 10.5
The Stimulus Editor utility
Stimulus files
The Stimulus Editor produces a file containing the stimuli with
their transient specification. These stimuli are defined as
simulator device declarations using the V (voltage source), I
(current source), and U STIM (digital stimulus generator)
forms. Since the Stimulus Editor produces these statements
automatically, you will never have to be concerned with their
syntax. However, if you are interested in a detailed description
of their syntax, see the descriptions of V and I devices in the
Analog Devices chapter and stimulus generator in the
Digital Devices chapter of the online PSpice Reference
Guide.
Configuring stimulus files
The Stimulus files list in the Configuration Files tab of the
Simulation Settings dialog box allows you to view the list of
stimulus files pertaining to your current schematic.
You can also manually add, delete, or change the stimulus file
configuration in this tab dialog box. The list box displays all of
the currently configured stimulus files. One file is specified per
line. Files can be configured as either global to the Capture
environment, local to the current design, or only for the current
profile. Global files are marked with the
icon before the file
name.
When starting the Stimulus Editor from Capture, stimulus files
are automatically configured (added to the list) as local to the
current design. Otherwise, new stimulus files can be added to
the list by entering the file name in the Filename text box and
then clicking the Add to Profile (profile specific configuration),
PSpice User's Guide
477
Chapter 12
Transient analysis
Product Version 10.5
Add to Design (local configuration) or Add as Global (global
configuration) button.
Starting the Stimulus Editor
The Stimulus Editor is fully integrated with Capture and can be
run from either the schematic editor or symbol editor.
You can start the Stimulus Editor by doing the following:
1
Select one or more stimulus instances in the schematic.
2
From the Edit menu, choose PSpice Stimulus.
When you first start the Stimulus Editor, you may need to
adjust the scale settings to fit the trace you are going to add.
You can use Axis Settings on the Plot menu or the
corresponding toolbar button to change the displayed data,
the extent of the scrolling region, and the minimum resolution
for each of the axes. Displayed Data Range parameters
determine what portion of the stimulus data set will be
presented on the screen. Extent of Scrolling Region
parameters set the absolute limits on the viewable range.
Minimum Resolution parameters determine the smallest
usable increment (example: if it is set to 1 msec, then you
cannot add a data point at 1.5 msec).
Defining stimuli
1
478
Place stimulus part instances from the symbol set:
VSTIM, ISTIM and DIGSTIMn (found in the
SOURCSTM.OLB part library).
PSpice User's Guide
Product Version 10.5
The Stimulus Editor utility
2
Click the source instance to select it.
3
From the Edit menu, choose PSpice Stimulus to start the
Stimulus Editor.
4
Fill in the transient specification according to the dialogs
and prompts.
Piecewise linear and digital stimuli can be specified by
direct manipulation of the input waveform display.
5
From the File menu, choose Save to save the edits.
6
Click Yes to update the schematic.
See Chapter 14, “Digital simulation,” for detailed information
about creating digital stimuli.
Example: piecewise linear stimulus
PSpice User's Guide
1
Open an existing schematic or start a new one.
2
From the Place menu, choose Part and browse the
SOURCSTM.OLB part library file for VSTIM (and select it).
3
Place the part. It looks like a regular voltage source with
an implementation property displayed.
4
Click the implementation label and type Vfirst. This
names the stimulus that you are going to create.
5
If you are working in a new schematic, choose Save from
the File menu. This schematic save step is necessary
since the schematic name is used to create the default
stimulus file name.
6
Click the VSTIM part to select it.
7
From the Edit menu, choose PSpice Stimulus. This starts
the Stimulus Editor and displays the New Stimulus dialog
479
Chapter 12
Transient analysis
Product Version 10.5
box. You can see that the stimulus already has the name
of Vfirst.
8
Select PWL in the dialog box and click OK. The cursor
looks like a pencil. The message in the status bar at the
bottom of the screen lets you know that you are in the
process of adding new data points to the stimulus. The
left end of the bottom status bar displays the current
coordinates of the cursor.
9
Move the cursor to (200ns, 1) and click the left mouse
button. This adds the point. Notice that there is
automatically a point at (0,0). Ignore it for now and
continue to add a couple more points to the right of the
current one.
10 Click-right to stop adding points.
11 From the File menu, choose Save.
If you make a mistake or want to make any changes, reshape
the trace by dragging any of the handles to a new location. The
dragged handle cannot pass any other defined data point.
To delete a point, click its handle and press Delete.
To add additional points, either choose Add Point from the Edit
menu, press Alt+A, or click the Add Point toolbar button
.
At this point you can return to Capture, edit the current
stimulus, or go on to create another.
480
PSpice User's Guide
Product Version 10.5
The Stimulus Editor utility
Example: sine wave sweep
This example creates a 10k sine wave with the amplitude
parameterized so that it can be swept during a simulation.
1
Open an existing schematic or start a new one.
2
Place a VSTIM part on your schematic.
3
To name the stimulus, double-click the implementation
property and type Vsin.
4
Click the VSTIM part to select it.
5
From the PSpice menu, choose Edit Stimulus to start the
Stimulus Editor.
6
Define the stimulus parameter for amplitude:
a. From the New Stimulus dialog box, choose Cancel.
b. From the Tools menu, choose Parameters.
c. Enter AMP=1 in the Definition text box, and click OK.
d. From the Stimulus menu, choose New or click the
New Stimulus button
in the toolbar.
e. Give the stimulus the name of Vsin.
f. Select SIN as the type of stimulus to be created, and
click OK.
7
PSpice User's Guide
Define the other stimulus properties:
481
Chapter 12
Transient analysis
Product Version 10.5
a. Enter 0 for Offset Value.
b. Enter {AMP} for Amplitude. The curly braces are
required. They indicate that the expression needs to
be evaluated at simulation time.
c. Enter 10k for Frequency and click OK.
d. From the File menu, choose Save.
e. Click Yes to update the schematic.
8
Within Capture, place and define the PARAM symbol:
a. From the Place menu, choose Part.
b. Either browse SPECIAL.OLB for the PARAM part or
type in the name.
c. Place the part on your schematic and double-click it.
d. Click New to add a new user property.
e. Set the value property name to AMP (no curly
braces).
f. Set the value of the AMP property to 1.
9
Set up the parametric sweep and other analyses:
a. From the PSpice menu, choose Edit Simulation
Profile, and select the Parametric Sweep option.
b. Select Global Parameter in the Swept Var. Type
frame.
c. Select Linear in the Sweep type frame.
10 Enter AMP in the Parameter name text box.
11 Specify values for the Start Value, End Value, and
Increment text boxes.
You can now set up your usual Transient, AC, or DC analysis
and run the simulation.
482
PSpice User's Guide
Product Version 10.5
The Stimulus Editor utility
Creating new stimulus symbols
1
PSpice User's Guide
Use the Capture part editor to edit or create a part with
the following properties:
Property
Value
Implementation
Type
PSpice Stimulus
Implementation
Name of the stimulus model
STIMTYPE
Type of stimulus; valid values are
ANALOG or DIGITAL; if this
property is nonexistent, the
stimulus is assumed to be
ANALOG
483
Chapter 12
Transient analysis
Product Version 10.5
Editing a stimulus
To edit an existing stimulus
1
Start the Stimulus Editor and select File, Open to open
the required Stimulus library.
2
Double-click the trace name (at the bottom of the X axis
for analog and to the left of the Y axis for digital traces.)
This opens the Stimulus Attributes dialog box where you
can modify the attributes of the stimulus directly and
immediately see the effect of the changes.
To edit a PWL stimulus
Note: PWL stimuli are a little different since they are a series
of time/value pairs.
1
Double-click the trace name. This displays the handles for
each defined data point.
2
Click any handle to select it. To reshape the trace, drag it
to a new location. To delete the data point, press Delete.
3
To add additional data points, either select Add from the
Edit menu or click the Add Point button.
4
Right-click to end adding new points.
To select a time and value scale factor for PWL stimuli
1
Select the PWL trace by clicking on its name.
2
Select Attributes from the Edit menu or click the
corresponding toolbar button
.
Note: The above procedure provides a fast way to scale a
PWL stimulus.
484
PSpice User's Guide
Product Version 10.5
The Stimulus Editor utility
Deleting and removing traces
To delete a trace from the displayed screen, select the trace
name by clicking on its name, then press Delete. This will only
erase the display of the trace, not delete it from your file. The
trace is still available by selecting Get from the Stimulus menu.
To remove a trace from a file, select Remove from the
Stimulus menu.
Note: Once a trace is removed, it is no longer retrievable.
Remove traces with caution.
Manual stimulus configuration
Stimuli can be characterized by manually starting the Stimulus
Editor and saving their specifications to a file. These stimulus
specifications can then be associated to stimulus instances in
your schematic or to stimulus symbols in the symbol library.
To manually configure a stimulus
1
Start the Stimulus Editor by choosing the Stimulus Editor
icon from the Windows Start menu, Release OrCAD 10.0
program group, PSpice Accessories option.
2
Open a stimulus file by choosing Open from the File
menu. If the file is not found in your current library search
path, you are prompted for a new file name.
3
Create one or more stimuli to be used in your schematic.
For each stimulus:
a. Name it whatever you want. This name will be used
to associate the stimulus specification to the stimulus
instance in your schematic, or to the symbol in the
symbol library.
b. Provide the transient specification.
c. From the File menu, choose Save.
4
PSpice User's Guide
In the schematic page editor, configure the Stimulus
Editor’s output file into your schematic:
485
Chapter 12
Transient analysis
Product Version 10.5
a. From the PSpice menu, choose Edit Simulation
Profile to display the Simulation Settings dialog box.
b. In the Simulation Settings dialog box, select the
Configuration Files tab.
c. Click Include in the Category field to display the
Include files list.
d. Enter the file name specified in step 2.
e. If the stimulus specifications are for only for the
current profile, click the Add to Profile button. For
local use in the current design, click the Add to
Design button. For global use by any design, use
Add as Global instead.
f. Click OK.
5
Modify either the stimulus instances in the schematic or
symbols in the symbol library to reference the new
stimulus specification.
6
Associate the transient stimulus specification to a
stimulus instance:
a. Place a stimulus part in your schematic from the part
set: VSTIM, ISTIM, and DIGSTIMn.
b. Click the VSTIM, ISTIM, or DIGSTIMn instance.
c. From the Edit menu, choose Properties.
d. Click the Implementation cell, type in the name of the
stimulus, and click Apply.
e. Complete specification of any VSTIM or ISTIM
instances by selecting Properties from the Edit menu
and editing their DC and AC attributes.
Click the DC cell and type its value.
Click the AC cell, type its value, and then click Apply.
f. Close the property editor spreadsheet.
7
486
To change stimulus references globally for a part:
PSpice User's Guide
Product Version 10.5
Transient (time) response
a. Select the part you want to edit.
b. From the Edit menu, choose Part to start the part
editor.
See Chapter 5, “Creating parts for models,” for a
description of how to create and edit parts.
c. Create or change the part definition, making sure to
define the following property:
Implementation
stimulus name as defined in
the Stimulus Editor
Finding out more about the Stimulus Editor
To find out more about
this...
See this...
Stimulus Editor
Stimulus Editor online help
Transient (time) response
The Transient response analysis causes the response of the
circuit to be calculated from TIME = 0 to a specified time. A
transient analysis specification is shown for the circuit
EXAMPLE.OPJ in Figure 12-1. (EXAMPLE.OPJ is shown in
Figure 12-2.)
PSpice User's Guide
487
Chapter 12
Transient analysis
Product Version 10.5
The analysis is to span the time interval from 0 to 1000
nanoseconds and values should be reported to the simulation
output file every 20 nanoseconds.
Figure 12-1 Transient analysis setup for
EXAMPLE.OPJ.
During a transient analysis, any or all of the independent
sources may have time-varying values. In EXAMPLE.OPJ, the
only source which has a time-varying value is V1 (VSIN part)
with attributes:
VOFF = 0v
VAMPL = 0.1v
FREQ = 5Meg
V1’s value varies as a 5 MHz sine wave with an offset voltage
of 0 volts and a peak amplitude of 0.1 volts.
488
PSpice User's Guide
Product Version 10.5
Transient (time) response
In general, more than one source has time-varying values; for
instance, two or more clocks in a digital circuit.
Figure 12-2 Example schematic EXAMPLE.OPJ.
Note: The example circuit EXAMPLE.OPJ is provided with
the PSpice program.
The transient analysis does its own calculation of a bias point
to start with, using the same technique as described for DC
sweep. This is necessary because the initial values of the
sources can be different from their DC values. In the
simulation output file EXAMPLE.OUT, the bias point report for
the transient bias point is labeled INITIAL TRANSIENT
SOLUTION. To report the bias point information for nonlinear
controlled sources and semiconductors, choose the OP
option from the Output File Options dialog box. This bias point
information is reported in the output file under the
OPERATING POINT INFORMATION section.
PSpice User's Guide
489
Chapter 12
Transient analysis
Product Version 10.5
Internal time steps in transient analyses
During analog analysis, PSpice maintains an internal time
step which is continuously adjusted to maintain accuracy
while not performing unnecessary steps. During periods of
inactivity, the internal time step is increased. During active
regions, it is decreased. The maximum internal step size can
be controlled by specifying it in the Maximum Time Step text
box in the Transient dialog box. PSpice will never exceed
either the step ceiling value or two percent of the total transient
run time, whichever is less.
The internal time steps used may not correspond to the time
steps at which information is reported. The values at the print
time steps are obtained by second-order polynomial
interpolation from values at the internal steps.
When simulating mixed analog/digital circuits, there are
actually two time steps: one analog and one digital. This is
necessary for efficiency. Since the analog and digital circuitry
usually have very different time constants, any attempt to lock
them together would greatly slow down the simulation. The
time step shown on the PSpice display during a transient
analysis is that of the analog section.
See Chapter 14, “Digital simulation,” for more information on the
digital timing analysis of PSpice A/D.
490
PSpice User's Guide
Product Version 10.5
Transient (time) response
Switching circuits in transient analyses
Running transient analysis on switching circuits can lead to
long run times. PSpice must keep the internal time step short
compared to the switching period, but the circuit’s response
extends over many switching cycles.
One method of avoiding this problem is to transform the
switching circuit into an equivalent circuit without switching.
The equivalent circuit represents a sort of quasi steady-state
of the actual circuit and can correctly model the actual circuit’s
response as long as the inputs do not change too fast.
This technique is described in: V. Bello, “Computer Program
Adds SPICE to Switching-Regulator Analysis,” Electronic
Design, March 5, 1981.
PSpice User's Guide
491
Chapter 12
Transient analysis
Product Version 10.5
Plotting hysteresis curves
Transient analysis can be used to look at a circuit’s hysteresis.
Consider, for instance, the circuit shown in Figure 12-3 (netlist
in Figure 12-4).
Figure 12-3 ECL-compatible Schmitt trigger.
* Capture Netlist
R_RIN
1 2 50
R_RC1
0 3 50
R_R1
3 5 185
R_R2
5 8 760
R_RC2
0 6 100
R_RE
4 8 260
R_RTH2
7 0 85
C_CLOAD 0 7 5PF
V_VEE
8 0 dc -5
V_VIN
1 0
+PWL 0 -8 1MS -1.0V 2MS -1.8V
R_RTH1
8 7 125
Q_Q1
3 2 4 QSTD
Q_Q2
6 5 4 QSTD
Q_Q3
0 6 7 QSTD
Q_Q4
0 6 7 QSTD
Figure 12-4 Netlist for Schmitt trigger circuit.
The QSTD model is defined as:
.MODEL QSTD NPN( is=1e-16 bf=50 br=0.1 rb=50 rc=10
tf=.12ns tr=5ns
+ cje=.4pF pe=.8 me=.4 cjc=.5pF pc=.8 mc=.333 ccs=1pF
va=50)
492
PSpice User's Guide
Product Version 10.5
Fourier components
Instead of using the DC sweep to look at the hysteresis, use
the transient analysis, (Print Step = .01ms and Final Time =
2ms) sweeping VIN from -1.8 volts to -1.0 volts and back down
to -1.8 volts, very slowly. This has two advantages:
■
it avoids convergence problems
■
it covers both the upward and downward transitions in
one analysis
After the simulation, in the Probe window in PSpice, the X axis
variable is initially set to Time. By selecting X Axis Settings
from the Plot menu and clicking on the Axis Variable button,
you can set the X axis variable to V(1). Then use Add on the
Trace menu to display V(7), and change the X axis to a
user-defined data range from -1.8V to -1.0V (Axis Settings on
the Plot menu). This plots the output of the Schmitt trigger
against its input, which is the desired outcome. The result
looks similar to Figure 12-5.
Figure 12-5 Hysteresis curve example: Schmitt trigger.
Fourier components
Fourier analysis is enabled through the Output File Options
dialog box under the Time Domain (Transient) Analysis type.
Fourier analysis calculates the DC and Fourier components of
the result of a transient analysis. By default, the first through
PSpice User's Guide
493
Chapter 12
Transient analysis
Product Version 10.5
ninth components are computed; however, more can be
specified.
Note: You must do a transient analysis in order to do a Fourier
analysis. The sampling interval used during the Fourier
transform is equal to the print step specified for the
transient analysis.
When selecting Fourier to run a harmonic decomposition
analysis on a transient waveform, only a portion of the
waveform is used. Using the Probe window in PSpice, a Fast
Fourier Transform (FFT) of the complete waveform can be
calculated and its spectrum displayed.
In the example shown in Figure 12-1 on page 488, the voltage
waveform at node OUT2 from the transient analysis is used
and the fundamental frequency is one megahertz for the
harmonic decomposition. The period of fundamental
frequency is one microsecond (inverse of the fundamental
frequency). Only the last one microsecond of the transient
analysis is used, and that portion is assumed to repeat
indefinitely. Since V1’s sine wave does indeed repeat every
one microsecond, this is sufficient. In general, however, you
must make sure that the fundamental Fourier period fits the
waveform in the transient analysis.
494
PSpice User's Guide
Monte Carlo and sensitivity/
worst-case analyses
13
Chapter overview
This chapter describes how to set up Monte Carlo and
sensitivity/worst-case analyses and includes the following
sections:
■
Statistical analyses on page 496
■
Monte Carlo analysis on page 506
■
Worst-case analysis on page 528
Note: This entire chapter describes features that are not
included in PSpice A/D Basics.
PSpice User's Guide
495
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Statistical analyses
Monte Carlo and sensitivity/worst-case are statistical
analyses. This section describes information common to both
types of analyses.
See Monte Carlo analysis on page 506 for information specific
to Monte Carlo analyses, and see Worst-case analysis on
page 528 for information specific to sensitivity/worst-case
analyses.
Note: Monte Carlo and sensitivity/worst-case analyses are
not included in PSpice A/D Basics.
Overview of statistical analyses
The Monte Carlo and worst-case analyses vary the lot or
device tolerances of devices between multiple runs of an
analysis (DC, AC, or transient). Before running the analysis,
you must set up the model and/or lot tolerances of the model
parameter to be investigated.
A Monte Carlo analysis performs a Monte Carlo (statistical)
analysis of the circuit. A worst-case analysis performs a
sensitivity and worst-case analysis of the circuit.
Sensitivity/worst-case analyses are different from Monte
Carlo analyses in that they compute the parameters using the
sensitivity data rather than using random numbers.
You can run either a Monte Carlo or a worst-case analysis, but
you cannot run both at the same time. Multiple runs of the
selected analysis are done while parameters are varied. You
can select only one analysis type (AC, DC, or transient) per
run. The selected analysis is repeated in subsequent passes
of the analysis.
Generating statistical results
As the number of Monte Carlo or worst-case runs increases,
simulation takes longer and the data file gets larger. Large
data files may be slow to open and slow to draw traces.
496
PSpice User's Guide
Product Version 10.5
Chapter overview
One way to work around this is to set up an overnight batch
job to run the simulation and execute commands. You can
even set up the batch job to produce a series of plots on paper
to be ready for you in the morning.
Output control for statistical analyses
Monte Carlo and sensitivity/worst-case analyses generate the
following types of reports:
■
Model parameter values used for each run (that is, the
values with tolerances applied)
■
Waveforms from each run, as a function of specifying
data collection, or by specifying output variables in the
analysis set up
■
Summary of all the runs using a collating function
Output is saved to the data file for use by the waveform
analyzer. For Monte Carlo analyses, you can use the
performance analysis feature to produce histograms of
derived data. For information about performance analysis, see
RLC filter example on page 459. For information about
histograms, see Creating histograms on page 523.
Model parameter values reports
To produce a list of the model parameters actually used for
each run,
1
In the Simulation Settings dialog box, click the Analysis
tab.
2
From the Analysis type list, select an analysis type.
3
Under Options, select Monte Carlo/Worst Case.
4
Click the More Settings button.
5
Select List model parameter values.
6
Click OK to close the Simulation Settings dialog box.
This list is written to the simulation output file at the beginning
of the run and contains the parameters for each device, as
PSpice User's Guide
497
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
opposed to the parameters for each .MODEL statement. This
is because devices can have different parameter values when
using a model statement containing a DEV tolerance.
Note that for midsize and large circuits, the List option can
produce a large output file.
Monte Carlo history support
Using the history support feature of Monte Carlo, you can
store the model parameter values used for each Monte Carlo
run, in a separate file, and later reuse these values.
For every Monte Carlo run, the model parameter values are
generated randomly with in the tolerance range specified by
you. With the history support feature, you can save these
randomly generated values and reuse exactly the same
values in the next analysis.
The Monte Carlo history support feature allows you to
compare the results of two Monte Carlo analyses by manually
changing only one or more parameter values. For comparison
between simulations, the random numbers have to remain the
same for the toleranced model parameters and this can be
achieved using the Monte carlo history support feature.
Saving parameter values in a file
To enable saving of the randomly generated model parameter
values:
1. Select PSpice > Edit Simulation Profile.
2. In the Simulation Settings dialog box, select the Analysis
tab.
3. Select the Analysis type as transient, DC or AC/Noise.
4. In the Options list select Monte Calro/Worst Case.
498
PSpice User's Guide
Product Version 10.5
Chapter overview
5. Select the MC Load/Save button.
6. In the Load/Save Monte Carlo Parameter File dialog box,
select the Save parameter values in filename: check
box.
7. In the text box that is enabled, specify the name and the
location of the file in which the parameter data is to be
saved.
8. Click OK to save your settings.
PSpice User's Guide
499
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
If you now run the Monte Carlo analysis, the model parameter
values used for various simulation runs will be stored in the
.mcp file specified by you.
Reusing parameter values
To reuse model parameter values from a previous Monte
Carlo analysis:
1. Select PSpice > Edit Simulation Profile.
2. In the Simulation Settings dialog box, select the Analysis
tab.
3. Select the Analysis type as transient, DC or AC/Noise.
4. In the Options list select Monte Calro/Worst Case.
5. Select the MC Load/Save button.
6. In the Load/Save Monte Carlo Parameter File dialog box,
select the Load parameter values in filename: check
box.
7. In the text box that is enabled, specify the name and the
location of the .mcp file from which the parameter data is
to be read.
8. Click OK to save your settings.
Now when you run the Monte Carlo analysis, the simulator will
reuse all the model parameter values stored in the .mcp files.
Any new or additional parameter values will be varied
separately with in the tolerance range.
While reusing values from a .mcp file, you must take care of
the points listed below.
1
500
When you use the Monte Carlo history support feature,
the values stored in a .mcp file for model parameters are
different from the values stored for components, such as
resistor, capacitor, and inductor. In case of model
parameters, actual parameter values used for simulation
are stored. Whereas in case of the components, instead
of the actual value, the multiplication factor used for
generating the random values are stored.
PSpice User's Guide
Product Version 10.5
Chapter overview
Table 13-1 on page 501 lists down the actual entries
recorded in a .mcp file for a model parameter and a
resistor.
Table 13-1 Entries in a .mcp file
For a model parameter:
base value 100
tolerance 10%
For a resistor:
base value 100
tolerance 10%
1.00000e+002
1
1.02747e+002
1.002
1.07986e+002
.986
1.04803e+002
1.003
9.17754e+001
.9912
The difference in the method used for storing values from
previous Monte Carlo runs, is highlighted when you
change the original value of a parameter and also choose
to reuse the values from a previous Monte Carlo run.
For example, if you change the original base value of a
model parameter from 100 to 50 and reuse the values
from an .mcp file, the simulation results will be based on
the original parameter value, which is 100. Whereas, in
case you change the value of a resistor from 100Ω to
10Ω , and reuse the values from a .mcp file, simulation
results will be based on the changed value of 10Ω .
2
If the number of Monte Carlo runs is greater than the
number of values in the .mcp file, PSpice simulator with
first reuse all the values from the .mcp file and then for
rest of the runs, the random values will be generated
using the base value and the tolerance defined for the
parameter in the schematic.
For example, consider that for a particular model
parameter, the .mcp file from which the parameter data
is to be read has 10 entries, but for the current simulation,
20 Monte Carlo runs are required. In such cases, for the
first 10 Monte Carlo runs the values will be read from the
.mcp file. For the last 10 runs, the simulator will calculate
PSpice User's Guide
501
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
the values using the base value of the model parameter
and the tolerance specified on it.
The Monte Carlo Parameter (.mcp) file
When you use the Monte Carlo history support feature, you
either generate a Monte Carlo Parameter (.mcp) file or use
parameters from a .mcp file. A .mcp file is a text file that
stores the parameter information generated during Monte
Carlo analysis. The data is stored in a tabular format with the
data values separated by white spaces, blanks, or tabs. Each
columns in a .mcp file indicates a parameter whose values
was varied during the Monte Carlo analysis.
The format for a .mcp file is shown below:
In a .mcp file, the name of the variable parameter is defined
using the following format:
<instance_name>::ParameterName.
502
where...
indicates...
instance_name
reference designator or the
name that appears in the
PSpice netlist
PSpice User's Guide
Product Version 10.5
Chapter overview
ParameterName
indicates whether the
component is a resistor,
capacitor, transistor, and so on.
For example, if the name of the variable parameter is
R_U2_R2::R, R_U2_R2 is the reference designator and R
indicates the parameter name, which in this case is a resistor.
A sample .mcp file that has three parameters values varied is
shown below.
Waveform reports
For Monte Carlo analyses, there are five variations of the
output that you can specify in the Save data from text box on
the Monte Carlo dialog box. Options:
<none>
All
First*
Every*
Runs(list)*
No output is generated
Forces all output to be generated (including
nominal run)
Generates output only during the first n runs
Generates output for every nth run
Does specified analysis and generates outputs
only for the listed runs (up to 25 values can be
specified in the list)
The * indicates that you can set the number of runs in the runs
text box.
Values for the output variables specified in the selected
analyses are saved to the simulation output file and data file.
PSpice User's Guide
503
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Note: In excess of about 10 runs, the waveform display can
look more like a band than a set of individual
waveforms. This can be useful for seeing the typical
spread for a particular output variable. As the number
of runs increases, the spread more closely
approximates the actual worst-case limits for the
circuit.
Note: Even a modest number of runs can produce large
output files.
Collating functions
You can further compress the results of Monte Carlo and
worst-case analyses. If you use the collating function, a single
number represents each run. (Click the More Settings Options
button and select a function from the Find list.) A table of
deviations per run is reported in the simulation output file.
Collating functions are listed in Table 13-2.
Table 13-2 Collating functions used in statistical
analyses
504
Function
Description
YMAX
Find the greatest difference in each
waveform from the nominal
MAX
Find the maximum value of each waveform
MIN
Find the minimum value of each waveform
RISE_EDGE
Find the first occurrence of the waveform
crossing above a specified threshold value
FALL_EDGE
Find the first occurrence of the waveform
crossing below a specified threshold value
PSpice User's Guide
Product Version 10.5
Chapter overview
Temperature considerations in statistical analyses
The statistical analyses perform multiple runs, as does the
temperature analysis. Conceptually, the Monte Carlo and
worst-case loops are inside the temperature loop.
However, since both temperature and tolerances affect the
model parameters, OrCAD recommends not using
temperature analysis when using Monte Carlo or worst-case
analysis.
Also, you cannot sweep the temperature in a DC sweep
analysis or put tolerances on temperature coefficients while
performing one of these statistical analyses. In
EXAMPLE.OPJ, the temperature value is fixed at 35 ° C.
Figure 13-1 Example schematic EXAMPLE.OPJ.
Note: The example schematic EXAMPLE.OPJ is provided
with the installed programs.
PSpice User's Guide
505
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Monte Carlo analysis
The Monte Carlo analysis calculates the circuit response to
changes in part values by randomly varying all of the model
parameters for which a tolerance is specified. This provides
statistical data on the impact of a device parameter’s variance.
Note: Monte Carlo analysis is not included in PSpice A/D
Basics.
Monte Carlo analysis is frequently used to predict yields on
production runs of a circuit. With Monte Carlo analysis, model
parameters are given tolerances, and multiple analyses (DC,
AC, or transient) are run using these tolerances.
For EXAMPLE.OPJ in Figure 13-1 on page 505, you can
analyze the effects of variances in the values of resistors RC1
and RC2 by assigning a model description to these resistors
that includes a 5% device tolerance on the multiplier
parameter R. The steps for adding the 5% device tolerance
are given below.
Then you can perform a Monte Carlo analysis. First, the
simulator performs a DC analysis with the nominal R multiplier
value for RC1 and RC2. Then it performs a set number of
additional runs with the R multiplier varied independently for
RC1 and RC2 within a 5% tolerance.
To modify example.opj and set up simulation
1
Replace RC1 and RC2 with RBREAK parts from the
BREAKOUT.OLB part library, setting property values to
match the resistors that are being replaced (VALUE=10k)
and reference designators to match previous names.
2
Select an RBREAK part and choose PSpice Model from
the Edit menu.
The Model Editor window appears.
3
Create the model CRES by replacing the model text:
.model Rbreak RES R=1
with the text:
506
PSpice User's Guide
Product Version 10.5
Chapter overview
.MODEL CRES RES( R=1 DEV=5% TC1=0.02
+ TC2=0.0045 )
Where TC1 is the linear temperature coefficient. TC2 is
the quadratic temperature coefficient.
4
From the File menu in Model Editor, choose Save.
The schematic editor automatically attaches the CRES
model to the selected RBREAK part by updating the
IMPLEMENTATION property on the part.
PSpice User's Guide
5
Double-click the second RBREAK part to display the
Parts spreadsheet.
6
In the IMPLEMENTATION text box, change the value to
CRES, then click Apply.
7
Close the Parts spreadsheet.
8
From the File menu, choose Save. By default, Capture
saves the definition to the model library EXAMPLE.LIB
and automatically configures the file for local use with the
current schematic.
9
In Capture, set up a new Monte Carlo analysis as shown
in Figure 13-2. The analysis specification tells PSpice to
507
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
do one nominal run and four Monte Carlo runs, saving the
DC analysis output from those five runs.
Figure 13-2 Monte Carlo analysis setup for EXAMPLE.OPJ.
Enter DC sweep settings in the Simulation Settings dialog box
Analysis tab.
1
Select Voltage source in the Sweep variable frame.
2
Enter V2 in the Name text box.
3
Select Linear in the Sweep type frame.
4
Enter a 0 in the Start value text box.
5
Enter a 12 in the End value text box.
6
Enter a 1 in the Increment text box.
PSpice starts by running all of the analyses enabled in the
Simulation Settings dialog box with all parameters set to their
nominal values.
508
PSpice User's Guide
Product Version 10.5
Chapter overview
However, with Monte Carlo enabled, PSpice saves the DC
sweep analysis results for later reference and comparison.
After the nominal analyses are finished, PSpice A/D performs
the additional specified analysis runs (in this example, DC
sweep).
Subsequent runs use the same analysis specification as the
nominal run with one major exception: instead of using the
nominal parameter values, the tolerances are applied to set
new parameter values and thus, new part values.
There is a trade-off in choosing the number of Monte Carlo
runs. More runs provide better statistics, but they require more
time. The amount of time scales directly with the number of
runs: 20 transient analyses take 20 times as long as one
transient analysis. During Monte Carlo runs, the PSpice status
display includes the current run number and the total number
of runs left.
Note: PSpice offers a facility to generate histograms of data
derived from Monte Carlo waveform families through
the performance analysis feature. For information
about performance analysis, see RLC filter example on
page 459. For information about histograms, see
Creating histograms on page 523.
History support
The Monte Carlo analysis calculates the circuit response to
changes in part values by randomly varying all of the model
parameters for which a tolerance is specified. However, at
times users might want to keep some or all of the parameters
similar for multiple analysis so that they can compare the
results of multiple simulations.
Consider an example of IC designs, which usually require
numerous runs. In such cases, rather than doing large number
of runs (with too many model parameters), users would prefer
doing less number of runs (with less number of parameters),
manually change some components/parameters values or
add a small amount of circuitry, and then continue the
analysis. Here user expects that simulator should use similar
values for all model parameters, so that a comparison can be
done between multiple simulations.
PSpice User's Guide
509
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
PSpice allows you to save randomly generated values for a
run in a .mcp file. You can then load this file to reuse the values
for subsequent runs.
Reading the summary report
The summary report generated in this example (see Figure
13-3) specifies that the waveform generated from V(OUT1)
should be the subject of the collating function YMAX. In each
of the last four runs, the new V(OUT1) waveform is compared
510
PSpice User's Guide
Product Version 10.5
Chapter overview
to the nominal V(OUT1) waveform for the first run, calculating
the maximum deviation in the Y direction (YMAX collating
function). The deviations are printed in order of size along with
their run number.
V(out1)
Figure 13-3 Summary of Monte Carlo runs for
EXAMPLE.OPJ.
With the List option enabled, a report is also generated
showing the parameter value used for each device in each
run. In this case (see Figure 13-4), run three shows the
highest deviation.
Figure 13-4 Parameter values for Monte Carlo
pass three.
PSpice User's Guide
511
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Example: Monte Carlo analysis of a pressure sensor
This example shows how the performance of a pressure
sensor circuit with a pressure-dependent resistor bridge is
affected by manufacturing tolerances, using Monte Carlo
analysis to explore these effects.
Drawing the schematic
To begin, construct the bridge as shown in Figure 13-5.
Figure 13-5 Pressure sensor circuit.
Here are a few things to know when placing and connecting
the part:
512
■
To get the part you want to place, from the Place menu,
choose Part.
■
To rotate a part before placing it, press R.
■
For V1 and Meter, place a generic voltage source using
the VSRC part. When you place the source for the meter,
change its name by double-clicking the part and typing
Meter in the Reference cell in the Parts Spreadsheet.
■
For R1-R7, place a resistor using the R part.
■
Place the analog ground using the 0 ground symbol from
the SOURCE.OLB part library.
PSpice User's Guide
Product Version 10.5
Chapter overview
■
To connect the parts, from the Place menu, choose Wire.
■
To move values or reference designators, click the value
or reference designator to select it, then drag it to the new
location.
Defining part values
Define the part values as shown in Figure 13-5. For the
pressure sensor, you need to do the following:
■
Change the resistor values for R3, R5, R6, and R7 from
their default value of 1 k.
■
Set the DC value for the V1 voltage source.
Note: Because the Meter source is used to measure current,
it has no DC value and can be left unchanged.
To change resistor values
1
Double-click the value for a resistor.
2
Type the new value. Depending on the resistor you are
changing, set its value to one of the following (refer to
Figure 13-5).
If you are changing
this resistor...
Type this...
R3
{1k*(1+P*Pcoeff/Pnom)}
Note: The value for R3—
{1k*(1+P*Pcoeff/Pnom)}
—is an expression that
represents linear
dependence of
resistance on pressure.
To complete the
definition for R3, you will
create and define global
parameters for Pcoeff, P,
and Pnom later on in this
example.
PSpice User's Guide
513
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
3
Product Version 10.5
If you are changing
this resistor...
Type this...
R5
2k
R6
470
R7
25
Repeat steps 1-2 for each resistor on your schematic
page.
To set the DC value for the V1 source and make it visible
1
Double-click the V1 source part.
2
In the Parts Spreadsheet, click in the cell under the DC
column.
3
Type 1.35v.
4
Click the Display button.
5
In the Display Format frame, choose the Value Only
option to make the DC value (1.35v) visible on the
schematic.
6
Click OK, then click Apply to apply the changes you have
made to the part.
7
Close the Parts Spreadsheet.
Setting up the parameters
To complete the value specification for R3, define the global
parameters Pcoeff, P, and Pnom.
To define and initialize Pcoeff, P, and Pnom
514
1
Place a PARAM part on the schematic page.
2
Double-click the PARAM part to display the Parts
Spreadsheet.
PSpice User's Guide
Product Version 10.5
Chapter overview
3
For each parameter, create a new property by clicking
New and typing its name. Enter its corresponding value
by clicking in the cell under the new property name and
typing its value. Specify the parameter name and
corresponding value as follows.
Table 13-3
4
Property
Value
Pcoeff
-0.06
P
0
Pnom
1.0
Click Apply to save the changes you have made then
close the Parts Spreadsheet.
Using resistors with models
To explore the effects of manufacturing tolerances on the
behavior of this circuit, you set device (DEV) and (LOT)
tolerances on the model parameters for resistors R1, R2, R3,
and R4 in a later step (see Defining tolerances for the resistor
models on page 516). This means you need to use resistor
parts that have model associations.
Because R parts do not have associated models (and
therefore no model parameters), change the resistor parts to
Rbreak parts that do have models.
Note: When PSpice A/D runs a Monte Carlo analysis, it uses
tolerance values to determine how to vary model
parameters during the simulation.
To replace R1, R2, R3, and R4 with the RBREAK part
PSpice User's Guide
1
Click R1 to select it.
2
Hold down the Ctrl key and click R2, R3 and R4 to add
them to the selection set.
3
Press Delete to delete the selection set.
515
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
4
From the Place menu, choose Part.
5
Type RBREAK in the Part text box. (If RBREAK is not
available, click the Add Library button and select
BREAKOUT.OLB to configure it for use in Capture.)
6
Click OK.
7
Manually place the RBREAK part in the circuit diagram
where R1, R2, R3 and R4 were located.
8
Double-click on each RBREAK part and change the
reference designators as desired.
Saving the design
Before editing the models for the Rbreak resistors, save the
schematic.
To save the design
1
From Capture’s File menu, choose Save.
Defining tolerances for the resistor models
This section shows how to assign device (DEV) and lot (LOT)
tolerances to the model parameters for resistors R1, R2, R3,
and R4 using the model editor.
You can use the model editor to change the .MODEL or
.SUBCKT syntax for a model definition. To find out more about
the model editor, see Editing model text on page 193, or refer
to the online PSpice Reference Guide.
To assign 2% device and 10% lot tolerances to the
resistance multiplier for R1
1
Select R1.
2
From the Edit menu, choose PSpice Model.
Capture searches the libraries for the Rbreak model
definition and makes a copy to create an instance model.
516
PSpice User's Guide
Product Version 10.5
Chapter overview
3
To change the instance model name from Rbreak to
Rmonte1, do the following:
a. In the Model Text frame, double-click Rbreak.
b. Type RMonte1.
4
To add a 2% device tolerance and a 10% lot tolerance to
the resistance multiplier, do the following:
a. Add the following to the .MODEL statement (after
R=1):
DEV=2% LOT=10%
The model editing window should look something
like Figure 13-6.
Figure 13-6 Model definition for RMonte1.
5
From the File menu, choose Save.
By default, Capture saves the RMonte1 .MODEL definition to
the DESIGN_NAME.LIB library, which is PSENSOR.LIB.
Capture also automatically configures the library for local use.
To find out more about adding model libraries to the
configuration, see Configuring model libraries on page 202.
PSpice User's Guide
517
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
To have resistors R2 and R4 use the same tolerances as
R1
1
In Capture’s schematic page editor, select R2 and R4.
2
From the Edit menu, select Properties.
3
In the R2 row, click in the cell under the Implementation
column and type RMonte1.
4
In the R4 row, click in the cell under the Implementation
column and type RMonte1.
To assign 5% device tolerance to the resistance multiplier for
R3
1
Select R3.
2
From the Edit menu, select PSpice Model.
3
In the Model Text frame, change the .MODEL statement
to:
.model RTherm RES R=1 DEV=5%
4
From the File menu, choose Save.
Your schematic page should look like Figure 13-7.
Setting up the analyses
This section shows how to define and enable a DC analysis
that sweeps the pressure value and a Monte Carlo analysis
that runs the DC sweep with each change to the resistance
multipliers.
To set up the DC sweep
1
In the PSpice menu, choose New Simulation Profile or
Edit Simulation Profile. (If this is a new simulation, enter
the name of the profile and click OK.)
The Simulation Settings dialog box appears.
See Setting up analyses on page 373 for a description of
the Simulation Settings dialog box.
518
PSpice User's Guide
Product Version 10.5
Chapter overview
Figure 13-7 Pressure sensor circuit with
RMonte1 and RTherm model definitions.
2
Select DC Sweep in the Analysis type list box.
3
In the Sweep Variable frame, select Global Parameter.
4
Enter the following values:
Table 13-4
In this text
box...
Type this...
Parameter
name
P
Start value
0
End value
5.0
Increment
0.1
To set up the Monte Carlo analysis
PSpice User's Guide
1
Select the Monte Carlo/Worst Case option.
2
Check Monte Carlo if it is not already selected.
3
In the Number of runs text box, type 10.
4
In the Save data from list box, select All.
5
Type I(Meter) in the Output variable text box.
519
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
6
Product Version 10.5
Click OK to save the simulation profile.
Running the analysis and viewing the results
To complete setup, simulate, and view results
1
From Capture’s PSpice menu, choose Run to start the
simulation
When the simulation is complete, PSpice automatically
displays the selected waveform. Because PSpice ran a
Monte Carlo analysis, it saved multiple runs or sections of
data. These are listed in the Available Sections dialog
box.
2
From PSpice’s Trace menu, choose Performance
Analysis.
3
Click the Select sections button.
4
In the Available Sections dialog box, click the All button.
5
Click OK.
6
To display current through the Meter voltage source, do
the following:
a. From Capture’s PSpice menu, point to markers and
choose Current into Pin.
b. Place a current probe on the left-hand pin of the
Meter source.
7
Switch to the Probe window to see the family of curves for
I(Meter) as a function of P.
Another way to view the family of curves without using
schematic markers is as follows:
a. From PSpice’s Trace menu, choose Add Trace.
b. In the Simulation Output Variables list, double-click
I(Meter).
Note: For more on analyzing Monte Carlo results in PSpice,
see the next section on Monte Carlo histograms.
520
PSpice User's Guide
Product Version 10.5
Chapter overview
Monte Carlo Histograms
You can display data derived from Monte Carlo waveform
families as histograms. This is part of the performance
analysis feature.
In this example, you simulate a fourth-order Chebyshev active
filter, running a series of 100 AC analyses while randomly
varying resistor and capacitor values for each run. Then,
having defined performance analysis measurements for
bandwidth and center frequency, you observe the statistical
distribution of these quantities for the 100 runs. For more
information about performance analysis, see RLC filter
example on page 459.
Chebyshev filter example
The Chebyshev filter is designed to have a 10 kHz center
frequency and a 1.5 kHz bandwidth. The schematic page for
the filter is shown in Figure 13-8. The stimulus specifications
for V1, V2, and V3 are:
V1: DC=-15
V2: DC=+15
V3: AC=1
The parts are rounded to the nearest available 1% resistor
and 5% capacitor value. In this example, note how the
PSpice User's Guide
521
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
bandwidth and the center frequency vary when 1% resistors
and 5% capacitors are used in the circuit.
Figure 13-8 Chebyshev filter.
Creating models for Monte Carlo analysis
To vary the resistors and capacitors in the filter circuit, create
models for these parts on which you can set device tolerances
for Monte Carlo analysis. The BREAKOUT.OLB library
contains generic devices for this purpose. The resistors and
capacitors in this schematic are the Rbreak and Cbreak parts
from BREAKOUT.OLB.
Using the Model Editor, modify the models for these parts as
follows:
.model RMOD RES(R=1 DEV=1%)
.model CMOD CAP(C=1 DEV=5%)
Setting up the analysis
To analyze the filter, set up both an AC analysis and a Monte
Carlo analysis. The AC analysis sweeps 50 points per decade
from 100 Hz to 1 MHz. The Monte Carlo analysis is set to take
100 runs. Save data from all runs and set the output variable
to V(OUT).
522
PSpice User's Guide
Product Version 10.5
Chapter overview
Creating histograms
Because the data file can become quite large when running a
Monte Carlo analysis, to view just the output of the filter, you
place a voltage probe at the output of the filter.
To collect data for the marked node only
1
From the PSpice menu, choose New Simulation Profile or
Edit Simulation Profile. (If this is a new simulation, enter
the name of the profile and click OK.)
The Simulation Settings dialog box appears.
2
On the Data Collection tab, choose the At Markers Only
option for each type of marker (Voltages, Currents,
Power, Digital, Noise).
3
Click OK.
To run the simulation and load Probe with data
1
From Capture’s PSpice menu, choose Run to start the
simulation.
When the simulation is complete, PSpice automatically
displays the selected waveform. Because PSpice ran a
Monte Carlo analysis, it saved multiple runs or sections of
data. These are listed in the Available Sections dialog
box.
2
In the Available Sections dialog box, click All.
3
Click OK.
To display a histogram for the 1 dB bandwidth
PSpice User's Guide
1
From PSpice’s Plot menu, choose Axis Settings.
2
Select the X Axis tab.
3
In the Processing Options frame, select the Performance
Analysis check box.
523
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
For information about performance analysis, see RLC
filter example on page 459.
4
Click OK.
The histogram display appears. The Y axis is the percent
of samples.
5
From the Trace menu, choose Add Trace.
6
Choose Bandwidth.
7
In the Trace Expression box, specify
Bandwidth(VDB(OUT),1).
Note: You can also display this histogram by using the
performance analysis wizard to display Bandwidth
(VDB(OUT),1).
To change the number of histogram divisions
1
From the Tools menu, choose Options.
2
In the Number of Histogram Divisions text box, replace 10
with 20.
3
Click OK.
The histogram for 1 dB bandwidth is shown in Figure 13-9.
Figure 13-9 1 dB bandwidth histogram.
524
PSpice User's Guide
Product Version 10.5
Chapter overview
The statistics for the histogram are shown along the bottom of
the display. The statistics show the number of Monte Carlo
runs, the number of divisions or vertical bars that make up the
histogram, mean, sigma, minimum, maximum, 10th
percentile, median, and 90th percentile.
■
Ten percent of the goal function values is less than or
equal to the 10th percentile number, and 90% of the goal
function values is greater than or equal to that number.
■
If there is more than one goal function value that satisfies
this criteria, then the 10th percentile is the midpoint of the
interval between the goal function values that satisfy the
criteria. Similarly, the median and 90th percentile
numbers represent goal function values such that 50%
and 90% (respectively) of the goal function values are
less than or equal to those numbers.
■
Sigma is the standard deviation of the goal function
values.
If needed, you can turn off the statistical data display as
follows:
1
From the Tools menu, choose Options.
2
Clear the Display Statistics check box.
3
Click Save, and then OK.
You can also show the distribution of the center frequency of
the filter.
To display the center frequency
1
From the Trace menu, choose Add Trace.
2
Choose CenterFreq.
3
In the Trace Expression box, specify
CenterFreq(VDB(OUT),1).
The new histogram replaces the previous histogram. To
display both histograms at once, choose Add Plot to Window
on the Plot menu before choosing Add from the Trace menu.
PSpice User's Guide
525
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
The histogram of the center frequency is as shown in Figure
13-10.
Figure 13-10 Center frequency histogram.
Copying histogram data
You can use the copy function to transfer the raw histogram
data points for a particular trace to the Windows clipboard.
This allows you to save the data as a standard ASCII text file,
or paste it directly into a report or other document for later
reference.
To copy histogram data to the clipboard
1
Select the trace symbol, or the trace name, in the
histogram.
2
From the Edit menu, choose Copy (or press Ctrl+C).
The histogram data points for the trace will be transfered
to the Windows clipboard.
To copy the histogram display to the clipboard
1
526
From the Window menu, choose Copy to Clipboard.
PSpice User's Guide
Product Version 10.5
Chapter overview
The histogram graph will be transfered to the Windows
clipboard.
PSpice User's Guide
527
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Worst-case analysis
This section discusses the analog worst-case analysis feature
of PSpice. The information provided in this section explains
how to use worst-case analysis properly and with realistic
expectations.
Note: Worst-case analysis is not included in PSpice A/D
Basics.
Overview of worst-case analysis
Worst-case analysis is used to find the worst probable output
of a circuit or system given the restricted variance of its
parameters. For instance, if the values of R1, R2, and R3 can
vary by +10%, then the worst-case analysis attempts to find
the combination of possible resistor values which result in the
worst simulated output. As with any other analysis, there are
three important parts: inputs, procedure, and outputs.
Inputs
In addition to the circuit description, you need to provide two
pieces of information:
■
the parameter tolerances
■
a definition of what worst means
You can set tolerances on any number of the parameters that
characterize a model.
Note: You can define models for nearly all primitive analog
circuit parts, such as resistors, capacitors, inductors,
and semiconductor devices. PSpice reads the standard
model parameter tolerance syntax specified in the
.MODEL statement. For each model parameter,
PSpice uses the nominal, minimum, and maximum
probable values, and the DEV and/or LOT specifiers;
the probability distribution type (such as UNIFORM or
GAUSS) is ignored.
528
PSpice User's Guide
Product Version 10.5
Chapter overview
The criterion for determining the worst values for the relevant
model parameters is defined in the .WC statement as a
function of any standard output variable in a specified range of
the sweep.
In a given range, reduce the measurement to a single value by
one of these five collating functions:
MAX
MIN
YMAX
RISE_EDGE
(value)
FALL_EDGE
(value)
Maximum output variable value
Minimum output variable value
Output variable value at the point where it
differs the most with the nominal run
Sweep value where the output variable
value crosses above a given threshold
value
Sweep value where the output variable
value crosses below a given threshold
value
You can define worst as the highest (HI) or lowest (LO)
possible collating function relative to the nominal run.
You can use analog behavioral models to measure waveform
characteristics other than those detected by the available
collating functions, such as rise time or slope. You can also
use analog behavioral models to incorporate several voltages
and currents into one output variable to which a collating
function may be applied. See Chapter 6, “Analog behavioral
modeling,” for more information.
Procedure
To establish the initial value of the collating function,
worst-case analysis begins with a nominal run using all model
parameters at their nominal values.
Next, multiple sensitivity analyses determine the individual
effect of each model parameter on the collating function. This
is accomplished by varying model parameters, one at a time,
in consecutive simulations. The direction (better or worse) in
which the collating function changes with a small increase in
each model parameter is recorded.
PSpice User's Guide
529
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Finally, for the worst-case run, each parameter value is taken
as far from its nominal as allowed by its tolerance, in the
direction which should cause the collating function to be its
worst (given by the HI or LO specification).
Note: This procedure saves time by performing the minimum
number of simulations required to make an educated
guess at the parameter values that produce the worst
results. It also has some limitations, which are
described in the following sections.
Outputs
A summary of the sensitivity analysis is printed in the PSpice
output file (.OUT). This summary shows the percent change
in the collating function corresponding to a small change in
each model parameter. If a .PROBE statement is included in
the circuit file, then the results of the nominal and worst-case
runs are saved for viewing in the Probe window.
Caution: An important condition for correct worst-case analysis
Worst-case analysis is not an optimization process; it does not
search for the set of parameter values that result in the worst
result.
It assumes that the worst case occurs when each parameter
has been either pushed to one of its limits or left at its nominal
value as indicated by the sensitivity analysis. It shows the true
worst-case results when the collating function is monotonic
within all tolerance combinations.
Otherwise, there is no guarantee. Usually you cannot be
certain whether this condition is true, but insight into the
operation of the circuit may alert you to possible anomalies.
530
PSpice User's Guide
Product Version 10.5
Chapter overview
Worst-case analysis example
The schematic shown in Figure 13-11 is for an amplifier circuit
that is a biased BJT. This circuit is used to demonstrate how a
simple worst-case analysis works. It also shows how
non-monotonic dependence of the output on a single
parameter can adversely affect the worst-case analysis.
Because an AC (small-signal) analysis is being performed,
setting the input to unity means that the output, Vm([OUT]), is
the magnitude of the gain of the amplifier. The only variable
declared in this circuit is the resistance of Rb2. Because the
value of Rb2 determines the bias on the BJT, it also affects the
amplifier’s gain.
Figure 13-11 Simple biased BJT amplifier.
Figure 13-12 is the circuit file used to run one of the following:
■
a parametric analysis (.STEP, shown enabled in the
circuit file) that sets the value of resistor Rb2 by stepping
model parameter R through values spanning the
specified DEV tolerance range, or
■
a worst-case analysis (shown disabled in the circuit file)
that allows PSpice to determine the worst-case value for
parameter R based upon a sensitivity analysis.
Only one of these analyses can run in any given simulation.
PSpice User's Guide
531
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Note: The AC and worst-case analysis specifications (.AC
and .WC statements) are written so that the worst-case
analysis tries to minimize Vm([OUT]) at 100 kHz.
The netlist and circuit file in Figure 13-12 are set up to run
either a parametric (.STEP) or worst-case (.WC) analysis of
the specified AC analysis. These simulations demonstrate the
conditions under which worst-case analysis works well and
those that can produce misleading results when output is not
monotonic with a variable parameter (see Figure 13-15 and
Figure 13-16).
* Worst-case analysis comparing monotonic and non-monotonic
* output with a variable parameter
.lib
***** Input signal and blocking capacitor *****
Vin In
0
ac
1
Cin In
B
1u
***** "Amplifier" *****
* gain increases with small increase in Rb2, but
* device saturates if Rb2 is maximized.
Vcc Vcc
0
10
Rc Vcc
C
1k
Q1 C
B
0
Q2N2222
Rb1 Vcc
B
10k
Rb2 B
0
Rbmod
720
.model Rbmod res(R=1 dev 5%)
; WC analysis results
; are correct
* .model Rbmod res(R=1.1 dev 5%)
; WC analysis misled
; by sensitivity
***** Load and blocking capacitor *****
Cout C
Out
1u
Rl Out
0
1k
* Run with either the .STEP or the .WC, but not both.
* This circuit file is currently set up to run the .STEP
* (.WC is commented out)
**** Parametric Sweep—providing plot of Vm([OUT]) vs. Rb2 ****
.STEP Res Rbmod(R) 0.8 1.2 10m
***** Worst-case analysis *****
* run once for each of the .model definitions stated above)
* WC AC Vm([Out]) min range 99k 101k list output all
.AC Lin 3 90k 110k
.probe
.end
Figure 13-12 Amplifier netlist and circuit file.
For demonstration, the parametric analysis is run first,
generating the curve shown in Figure 13-15 and Figure 13-16.
532
PSpice User's Guide
Product Version 10.5
Chapter overview
This curve, derived using the YatX goal function shown in
Figure 13-14 illustrates the non-monotonic dependence of
gain on Rb2.
YatX(1, X_value)=y1{1|sfxv(X_value)!1;}
Figure 13-13 YatX Goal Function
To do this yourself, place the goal function definition in a
PROBE.GF file in the circuit directory. Then start PSpice, load
all of the AC sweeps, set up the X axis for performance
analysis, and add the following trace:
YatX(Vm([OUT]),100k)
Note: The YatX goal function is used on the simulation results
for the parametric sweep (.STEP) defined in Figure
13-12. The resulting curves are shown in Figure 13-15
and Figure 13-16.
Next, the parametric analysis is commented out and the
worst-case analysis is enabled. Two runs are made using the
two versions of the Rbmod .MODEL statement shown in the
circuit file. The model parameter, R, is a multiplier which is
used to scale the nominal value of any resistor referencing the
Rbmod model (Rb2 in this case).
The first .MODEL statement leaves the nominal value of Rb2
at 720 ohms. The sensitivity analysis increments R by a small
amount and checks its effect on Vm([OUT]). This slight
increase in R causes an increase in the base bias voltage of
the BJT, and increases the amplifier’s gain, Vm([OUT]). The
worst-case analysis correctly sets R to its minimum value for
the lowest possible Vm([OUT]) (see Figure 13-15).
The second .MODEL statement scales the nominal value of
Rb2 by 1.1 to approximately 800 ohms. The gain still
increases with a small increase in R, but a larger increase in
R increases the base voltage so much that it drives the BJT
into saturation and nearly eliminates the gain. The worst-case
analysis is fooled by the sensitivity analysis into assuming that
Rb2 must be minimized to degrade the gain, but maximizing
Rb2 is much worse (see Figure 13-16). Note that even an
PSpice User's Guide
533
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
optimizer, which checks the local gradients to determine how
the parameters should be varied, is fooled by this circuit.
Figure 13-15 Correct worst-case results.
In the above figure, output is monotonic within the tolerance
range. Sensitivity analysis correctly points to the minimum
value.
Figure 13-16 Incorrect worst-case results.
In the above figure, output is non-monotonic within the
tolerance range, thus producing incorrect worst-case results.
Consider a slightly different scenario: Rb2 is set to 720 ohms
so that maximizing it is not enough to saturate the BJT, but
534
PSpice User's Guide
Product Version 10.5
Chapter overview
Rb1 is variable also. The true worst case occurs when Rb2 is
maximized and Rb1 is minimized. Checking their individual
effects is not sufficient, even if the circuit were simulated four
times with each resistor in turn set to its extreme values.
Tips and other useful information
VARY BOTH, VARY DEV, and VARY LOT
When VARY BOTH is specified in the .WC statement and a
model parameter is specified with both DEV and LOT
tolerances defined, the worst-case analysis may produce
unexpected results. The sensitivity of the collating function is
only tested with respect to LOT variations of such a parameter.
Figure 13-17 Schematic
using VARY BOTH.
For example, during the sensitivity analysis, the parameter is
varied once affecting all devices referring to it and its effect on
the collating function is recorded. For the worst-case analysis,
the parameter is changed for all devices by LOT + DEV in the
determined direction. See the example schematic in Figure
13-17 and circuit file in Figure 13-18.
WCASE VARY BOTH
Vin
Rs
Rwc1
Rwc2
.MODEL Rmod
.DC Vin
.WC DC
.ENDS
PSpice User's Guide
Test
1
0
10V
1
2
1K
2
3
Rmod
100
3
0
Rmod
100
RES(R=1 LOT 10% DEV 5%)
LIST
10
V(3)
MAX
VARY BOTH
LIST
OUTPUT ALL
535
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Figure 13-18 Circuit file using VARY BOTH.
In this case, V(3) is maximized if:
■
Rwc1 and Rwc2 are both increased by 10% per the LOT
tolerance specification, and
■
Rwc1 is decreased by 5% and Rwc2 is increased by 5%
per the DEV tolerance specification.
The final values for Rwc1 and Rwc2 should be 105 and 115,
respectively. However, because Rwc1 and Rwc2 are varied
together during the sensitivity analysis, it is assumed that both
must be increased to their maximum for a maximum V(3).
Therefore, both are increased by 15%.
The purpose of the technique is to reduce the number of
simulations. For a more accurate worst-case analysis, you
should first perform a worst-case analysis with VARY LOT,
manually adjust the nominal model parameter values
according to the results, then perform another analysis with
VARY DEV specified.
Gaussian distributions
Parameters using Gaussian distributions are changed by 3σ
(three times sigma) for the worst-case analysis.
YMAX collating function
The purpose of the YMAX collating function is often
misunderstood. This function does not try to maximize the
deviation of the output variable value from nominal.
Depending on whether HI or LO is specified, it tries to
maximize or minimize the output variable value itself at the
point where maximum deviation occurred during sensitivity
analysis.
Note: This may result in maximizing or minimizing the output
variable value over the entire range of the sweep. This
collating function is useful when you know the direction
in which the maximum deviation occurs.
536
PSpice User's Guide
Product Version 10.5
Chapter overview
RELTOL
During the sensitivity analysis, each parameter is varied
(multiplied) by 1+RELTOL where RELTOL is specified in a
.OPTIONS statement, or defaults to 0.001.
Sensitivity analysis
The sensitivity analysis results are printed in the output file
(.OUT). For each varied parameter, the percent change in the
collating function and the sweep variable value at which the
collating function was measured are given. The parameters
are listed in worst output order; for example, the collating
function was its worst when the first parameter printed in the
list was varied.
When you use the YMAX collating function, the output file also
lists mean deviation and sigma values. These are based on
the changes in the output variable from nominal at every
sweep point in every sensitivity run.
Manual optimization
You can use worst-case analysis to perform manual
optimization with PSpice. The monotonicity condition is
usually met if the parameters have a very limited range.
Performing worst-case analysis with tight tolerances on the
parameters produces sensitivity and worst-case results (in the
output file). You can use these to decide how the parameters
should be varied to achieve the desired response. You can
then make adjustments to the nominal values in the circuit file,
and perform the worst-case analysis again for a new set of
gradients.
Note: Parametric sweeps (.STEP), like the one performed in
the circuit file shown in Figure 13-12, can be used to
augment this procedure.
PSpice User's Guide
537
Chapter 13
Monte Carlo and sensitivity/worst-case analyses
Product Version 10.5
Monte Carlo analysis
Monte Carlo (.MC) analysis may be helpful when worst-case
analysis cannot be used. Monte Carlo analysis can often be
used to verify or improve on worst-case analysis results.
Monte Carlo analysis randomly selects possible parameter
values, which can be thought of as randomly selecting points
in the parameter space. The worst-case analysis assumes
that the worst results occur somewhere on the surface of this
space, where parameters (to which the output is sensitive) are
at one of their extreme values.
If this is not true, the Monte Carlo analysis may find a point at
which the results are worse. To try this, replace .WC in the
circuit file with .MC <#runs>, where <#runs> is the number of
simulations you want to perform. More runs provide higher
confidence results. The Monte Carlo summary in the output
file lists the runs in decreasing order of collating function
value.
Tip
To save disk space, do not specify any OUTPUT
options.
Next, add the following option to the .MC statement, and
simulate again.
OUTPUT LIST RUNS <worst_run#>
This performs only two simulations: the nominal and the worst
Monte Carlo run. The parameter values used during the worst
run are written to the output file, and the results of both
simulations are saved.
Using Monte Carlo analysis with YMAX is a good way to
obtain a conservative guess at the maximum possible
deviation from nominal, since worst-case analysis usually
cannot provide this information.
538
PSpice User's Guide
Digital simulation
14
Chapter overview
This chapter describes how to set up a digital simulation
analysis and includes the following sections:
■
What is digital simulation? on page 540
■
Steps for simulating digital circuits on page 540
■
Concepts you need to understand on page 541
■
Defining a digital stimulus on page 543
■
Defining simulation time on page 558
■
Adjusting simulation parameters on page 558
■
Starting the simulation on page 562
■
Analyzing results on page 563
Note: This entire chapter describes features that are not
included in PSpice.
PSpice User's Guide
539
Chapter 14
Digital simulation
Product Version 10.5
What is digital simulation?
Digital simulation is the analysis of logic and timing behavior
of digital devices over time. PSpice A/D simulates this
behavior during transient analysis. When computing the bias
point, PSpice A/D considers the digital devices in addition to
any analog devices in the circuit.
PSpice A/D performs detailed timing analysis subject to the
constraints specified for the devices. For example, flip-flops
perform setup checks on the incoming clock and data signals.
PSpice A/D reports any timing violations or hazards as
messages written to the simulation output file and the
waveform data file. See Tracking timing violations and hazards
on page 569 for information about persistent hazards, and for
descriptions of the warning messages.
Steps for simulating digital circuits
There are six steps in the development and simulation of
digital circuits:
1
Drawing the design.
For more information on drawing designs see your
OrCAD Capture User’s Guide. Steps 2 through 6 of
this process are covered in this chapter.
540
2
Defining the stimuli.
3
Setting the simulation time.
4
Adjusting the simulation parameters.
5
Starting the simulation.
6
Analyzing the results.
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
Concepts you need to understand
States
When the circuit is in operation, digital nodes take on values
or output states shown in Table 14-1. Each digital state has a
strength component as well. Strengths are described in the
next section.
Table 14-1 Digital states
This
state...
Means this...
0
Low, false, no, off
1
High, true, yes, on
R
Rising (changes from 0 to 1 sometime
during the R interval)
F
Falling (changes from 1 to 0 sometime
during the F interval)
X
Unknown: may be high, low, intermediate,
or unstable
Z
High impedance: may be high, low,
intermediate, or unstable
Note: States do not necessarily correspond to a specific, or
even stable, voltage. A logical 1 level means only that
the voltage is somewhere within the high range for the
particular device family. The rising and falling levels
only indicate that the voltage crosses the 0–1 threshold
at some time during the R or F interval, not that the
voltage change follows a particular slope.
PSpice User's Guide
541
Chapter 14
Digital simulation
Product Version 10.5
Strengths
When a digital node is driven by more than one device,
PSpice A/D determines the correct level of the node. Each
output has a strength value, and PSpice A/D compares the
strengths of the outputs driving the node. The strongest
driver determines the resulting level of the node. If outputs of
the same strength but different levels drive a node, the node’s
level becomes X.
PSpice A/D supports 64 strengths. The lowest (weakest)
strength is called Z. The highest (strongest) strength is called
the forcing strength. The Z strength (called high impedance)
is typically output by disabled tristate gates or open-collector
output devices. PSpice A/D reports any nodes of Z strength
(at any level) as Z, and reports all other nodes by the
designations shown in Digital states on page 541.
For additional information on this topic see Defining Output
Strengths on page 350 of Chapter 7, “Digital device
modeling.”
542
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
Defining a digital stimulus
A digital stimulus defines input to the digital portions of your
circuit, playing a role similar to that played by the independent
voltage and current sources for the analog portion of your
circuit.
The following table summarizes the digital stimuli provided in
the part libraries.
Table 14-2
If you want to
specify the
input signal by...
Then use this
part...
For this type of
digital input...
Using the Stimulus DIGSTIMn
Editor1
signal or bus stimulus
Defining part
properties
DIGCLOCK
clock signal
STIM1
one-bit stimulus
STIM4
four-bit stimulus
STIM8
eight-bit stimulus
STIM16
sixteen-bit stimulus
FILESTIM1
one-bit file-based
stimulus
FILESTIM2
two-bit file-based
stimulus
FILESTIM4
four-bit file-based
stimulus
FILESTIM8
eight-bit file-based
stimulus
FILESTIM16
sixteen-bit file-based
stimulus
FILESTIM32
thirty-two-bit
file-based stimulus
1. Stimulus Editor is not included with PSpice A/D Basics
PSpice User's Guide
543
Chapter 14
Digital simulation
Product Version 10.5
Using the DIGSTIMn part
Use the DIGSTIMn stimulus parts to define a stimulus for a net
or bus using the Stimulus Editor.
Note: Stimulus Editor is not included with PSpice A/D Basics.
To use the DIGSTIMn part
1
From Capture’s Place menu, choose Part.
2
Place and connect the DIGSTIM1 stimulus part from
SOURCSTM.OLB to a wire or bus in your design.
3
Click the stimulus instance to select it.
4
From the Edit menu, choose PSpice Stimulus.
This starts the Stimulus Editor. The New Stimulus dialog
box appears prompting you to define a new stimulus.
5
Enter DIGSTIM1 in the Name text box.
6
In the Digital frame, select Signal.
7
Click OK.
8
Define stimulus transitions; see Defining input signals
using the Stimulus Editor below.
Defining input signals using the Stimulus Editor
Note: Stimulus Editor is not included with PSpice A/D Basics.
Defining signal transitions
You can do any of the following when defining digital signal
transitions:
544
■
Add a transition
■
Move a transition
■
Edit a transition
■
Delete a transition
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
Note: These operations cannot be applied to a stimulus
defined as a clock signal.
To add a transition
1
From the Plot menu, choose Axis Settings.
2
Enter values in the Displayed Range for Time text boxes
and the Timing Resolution text box as required for adding
transitions.
For example, if you wish to add transitions every 1ms, set
the Timing Resolution to 1ms.
3
Select the digital stimulus you want to edit.
When you select a transition to edit, a red handle
appears.
4
From the Stimulus Editor’s Edit menu, choose Add.
5
Click the waveform at the time where the transition is
required.
6
Repeat step 4 to add additional transitions.
7
When you finish, right-click to exit the edit mode.
To move a transition
1
Click the transition you want to move.
2
If needed, use Shift+click to select additional transitions
on the same signal or different signals.
3
Reposition the transition (or transitions) by dragging.
Note: If you press Shift while dragging, then all selected
transitions move by the same amount.
To edit a transition
1
Do one of the following:
❑
PSpice User's Guide
Select the transition you want to edit and from the
Edit menu, choose Attributes.
545
Chapter 14
Digital simulation
Product Version 10.5
❑
Double-click the transition you want to edit.
2
In the Edit Digital Transition dialog box, edit the timing and
value of the transition.
3
Click OK.
To delete a transition
1
Click the transition you want to delete.
2
If needed, press Shift+click to select additional
transitions on the same signal or different signals.
3
From the Edit menu, choose Delete.
Defining clock transitions
To create a clock stimulus
1
In the Stimulus Editor, select the stimulus that you want to
use as a clock.
2
From the Stimulus menu, choose Change Type.
3
Under Type, choose Clock.
4
Click OK.
5
Enter values for the clock signal attributes as described
below.
Table 14-3
546
For this
attribute...
Enter this...
Frequency
clock rate
Duty Cycle
percent of high versus low in
decimal or integer units
Initial Value
starting value: 0 or 1
Time Delay
time after simulation begins
when the clock stimulus takes
effect
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
Example: To create a clock signal with a clock rate of 20
MHz, 50% duty cycle, a starting value of 1, and time delay
of 5 nsec, set the signal properties as follows:
Frequency
Duty Cycle
Initial Value
Time Delay
6
=
=
=
=
20Meg
0.50 (or 50)
1
5ns
From the File menu, choose Save.
Note: If you have the PSpice A/D Basics package, you can
define clock signals using DIGCLOCK. To find out
more, see Using the DIGCLOCK part on page 552.
To change clock attributes
1
In the Stimulus Editor, do one of the following:
❑
Double-click the clock name to the left of the axis.
❑
Click the clock name and from the Edit menu, choose
attributes.
2
Modify the clock attributes as needed.
3
Click OK.
Defining bus transitions
There are three steps for creating a bus:
1
Creating the digital bus stimulus.
2
Introducing transitions.
3
Optionally defining the radix for bus values.
These steps are described in detail in the following
procedures.
To create a digital bus stimulus
PSpice User's Guide
1
From the Stimulus menu, choose New.
2
In the Name text box, enter Bus.
547
Chapter 14
Digital simulation
Product Version 10.5
3
In the Digital frame, select Bus.
4
If needed, change the bus width from its default value of
8 bits. To do this, in the Width text box, type a different
integer.
5
Click OK.
During any interval, the bits on the bus lines represent a value
from zero through (2n - 1), where n is the number of bus lines.
To set bus values, introduce transitions using either of the two
methods described below.
To introduce transitions (method one)
1
From the Plot menu, choose Axis Settings.
2
Enter values in the Displayed Range for Time text boxes
and the Timing Resolution text box as required for adding
transitions.
For example, if you wish to add transitions every 1 ms, set
the Timing Resolution to 1ms.
3
From the Stimulus Editor’s Edit menu, choose Add.
4
In the digital value field on the toolbar (just right of the Add
button), type a bus value in any of the following ways:
Table 14-4
To get this
effect...
Type this...
A literal value
<unsigned_number>[;radix]
Example: 12
An increment
+<unsigned_number>[;radix]
Example: +12;H
A decrement
-<unsigned_number>[;radix]
Example: -12;O
548
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
If you do not enter a radix value, the Stimulus Editor
appends the default bus radix. To find out about valid
radix values, see page 14-11.
5
Click the waveform where you want the transition added.
6
Repeat steps 4 and 5 as needed.
7
When you finish, right-click to exit the editing mode.
To introduce transitions (method two)
1
From the Plot menu, choose Axis Settings.
2
Enter values in the Dislayed Range for Time text boxes
and the Timing Resolution text box as required for adding
transitions.
For example, if you wish to add transitions every 1 ms, set
the Timing Resolution to 1ms.
3
From the Stimulus Editor’s Edit menu, choose Add.
4
Place the tip of the pencil-shaped pointer on the
waveform, and click to create transitions as shown
here:
Here are some other things that you can do:
PSpice User's Guide
❑
Move a transition left or right by clicking and
dragging.
❑
Delete a transition by selecting it and then, from the
Edit menu, choosing Delete (or by pressing Del).
❑
Select more than one transition by holding down
Shift while clicking.
5
When you finish creating transitions, right-click.
6
Click the transition at the start (far left) of the interval. A
small diamond appears over the transition.
549
Chapter 14
Digital simulation
Product Version 10.5
7
From the Edit menu, choose Attributes to display the Edit
Digital Transition dialog box.
8
In the Transition Type frame, choose Set Value,
Increment, or Decrement.
9
Do one of the following to specify the bus value:
❑
In the Value text box, type a value.
❑
Select one of these defaults from the list: 0, All bits 1,
X (Unknown), or Z (High impedance).
10 Click OK.
11 Repeat steps 6 through 10 for each transition.
To set the default bus radix
1
From the Tools menu, choose Options.
2
In the Bus Display Defaults frame, from the Radix list,
select the radix you want as default.
Table 14-5
3
550
Select this
radix...
To show values in this
notation...
Binary
base 2
Octal
base 8
Decimal
base 10
Hexadecimal
base 16
Click OK.
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
Adding loops
Suppose you have a stimulus that looks like this:
A
B
and you want to create a stimulus that consists of three
consecutive occurrences of the sequence that starts at A and
ends at B:
You can do this by using a standard text editor to edit a
stimulus library file. Within this file is a sequence of transitions
that produces the original waveform. With a text editor you can
modify the stimulus definition so it repeats itself.
To add a loop
1
In the Stimulus Editor, save and close the stimulus file.
2
In a standard text editor (such as Notepad), open the
stimulus file.
3
Find the set of consecutive lines comprising the
sequence that you want to repeat.
Each relevant line begins with the time of the transition
and ends with a value or change in value.
To find out more about the syntax of the stimulus
commands used in the stimulus file, refer to the online
PSpice Reference Guide.
4
Before these lines, insert a line that uses this syntax:
+ Repeat for n_times
where n_times is one of the following:
❑
PSpice User's Guide
A positive integer representing the number of
repetitions.
551
Chapter 14
Digital simulation
Product Version 10.5
The keyword FOREVER, which means repeat this
sequence for an unlimited number of times (like a
clock signal).
❑
5
Below these lines, insert a line that uses this syntax:
+ Endrepeat
6
From the File menu, choose Save.
Given the example shown on page 3, if you wanted to repeat
the sequence shown from point A to point B three times, then
you would modify the stimulus file as shown here (added lines
are in bold):
+
+
+
+
+
+
+
Repeat for 3
+0s 000000000
250us INCR BY 000000001
500us 000000010
750us INCR BY 000000001
1ms 000000000
Endrepeat
Using the DIGCLOCK part
The DIGCLOCK part allows you to define a clock signal by
using the part’s properties.
For information on how to define a clock signal using the
Stimulus Editor with the DIGSTIMn part, see Defining signal
transitions on page 544.
To define a clock signal using DIGCLOCK
1
From Capture’s Place menu, choose Part.
2
Place and connect a DIGCLOCK part.
3
Double-click the part instance.
4
Define the properties as described below.
Table 14-6
For this property... Specify this...
DELAY
552
Time before the first transition of the
clock
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
Table 14-6
For this property... Specify this...
ONTIME
Time in high state for each period
OFFTIME
Time in low state for each period
STARTVAL
Low state of clock (default:0)
OPPVAL
High state of clock (default: 1)
Using STIM1, STIM4, STIM8 and STIM16 parts
The STIMn parts have a single pin for connection. STIM1 is
used for driving a single net. STIM4, STIM8 and STIM16 drive
buses that are 4, 8 and 16 bits wide, respectively. The
properties for all of these parts are the same as those shown
in Table 14-7 below.
Table 14-7
PSpice User's Guide
Property
Description
WIDTH
Number of output signals (nodes).
FORMAT
Sequence of digits defining the number of
signals corresponding to a digit in any
<value> term appearing in a COMMANDn
property definition. Each digit must be
either 1, 3, or 4 (binary, octal,
hexadecimal, respectively); the sum of all
digits in FORMAT must equal WIDTH.
IO_MODEL
I/O model describing the stimulus’ driving
characteristics.
IO_LEVEL
Interface subcircuit selection from one of
the four analog/digital subcircuits provided
with the part’s I/O model.
DIG_PWR
Digital power pin used by the interface
subcircuit.
DIG_GND
Digital ground pin used by the interface
subcircuit.
553
Chapter 14
Digital simulation
Product Version 10.5
Table 14-7
Property
Description
TIMESTEP
Number of seconds per clock cycle or
step.
COMMAND1COMMAND16
Stimulus transition specification
statements including time/value pairs,
labels, and conditional constructs.
When placed, you must connect each part to the wire or bus
of the corresponding radix. Generally, you only need to modify
the FORMAT, TIMESTEP, and COMMANDn properties.
Typically, each COMMANDn property contains only one
command line. It is possible to enter more than one command
line per property by placing \n+ between command lines in a
given definition. (The n must be lower case and no spaces
between characters; spaces may precede or follow the entire
key sequence.) Refer to the online PSpice Reference Guide
for information about command line syntax.
Using the FILESTIMn parts
The FILESTIMn parts have a single pin for connection to the
rest of the circuit. FILESTIM1 is used for driving a single net.
FILESTIM2, FILESTIM4, FILESTIM8, FILESTIM16 and
FILESTIM32 drive buses that are 2, 4, 8, 16 and 32 bits wide,
respectively. You must define the digital stimulus specification
in an external file. Using this technique, stimulus definitions
can be created from scratch or extracted with little
modification from another simulation’s output file. Refer to the
online PSpice Reference Guide for more information about
creating digital stimulus specifications and files.
Table 14-8 lists the properties of the FILESTIMn parts. The
IO_MODEL, IO_LEVEL, and PSPICEDEFAULTNET
properties describing this part’s I/O characteristics are
provided with default values that rarely need modification.
However, you must define the FILENAME property with the
name of the external file containing the digital stimulus
specification.
554
PSpice User's Guide
Product Version 10.5
Steps for simulating digital circuits
The SIGNAME property specifies the name of the signal
inside the stimulus file which becomes the output from the
FILESTIMn part. If left undefined, the name of the connected
net (generally a labeled wire) determines which signal is used.
Table 14-8 FILESTIMn part properties
Property
Description
FILENAME
Name of file containing the
stimulus specification.
Note: If you do not specify the path
to the stimulus file, you must
place the file in the folder for
the simulation profile for
which you are configuring
the stimulus.
PSpice User's Guide
SIGNAME
Name of output signal
IO_MODEL
I/O model describing the stimulus’
driving characteristics
IO_LEVEL
Interface subcircuit selection from
one of the four AtoD or DtoA
subcircuits provided with the part’s
I/O model
PSPICEDEFAULTNET
Hidden digital power and ground
pins used by the interface
subcircuit. Name of the default net
to use.
555
Chapter 14
Digital simulation
Product Version 10.5
For example, a FILESTIMn part can be used to reset a
counter, which could appear as shown in Figure 14-1 below.
Figure 14-1 FILESTIM1 used on a schematic
page.
In this case, the FILESTIM1 part instance, U2, generates a
reset signal to the CLR pin of the 74393 counter.
To set up the U2 stimulus
The following steps set up the U2 stimulus so that the 74393
counter is cleared after 40 nsec have elapsed in a transient
analysis.
1
Create a stimulus file named RESET.STM that contains
the following lines:
Reset
0ns 1
40ns 0
The header line contains the names of all signals
described in the file. In this case, there is only one: Reset.
The remaining lines are the state transitions output for the
signals named in the header. In this case, the Reset
signal remains at state 1 until 40nsec have elapsed, at
which time it drops to state 0.
Note: A blank line is required between the signal name
list and the first transition.
2
556
Place the RESET.STM file in the folder for the simulation
profile for which you are configuring the stimulus.
PSpice User's Guide
Product Version 10.5
PSpice User's Guide
Steps for simulating digital circuits
3
Associate this file with the digital stimulus instance, U2,
by setting U2’s FILENAME property to RESET.STM.
4
Define the signal named Reset in RESET.STM as the
output of U2 by setting U2’s SIGNAME property to Reset.
Since the labeled wire connecting U2 with the 74393
counter is also named Reset, it is also acceptable to leave
SIGNAME undefined.
557
Chapter 14
Digital simulation
Product Version 10.5
Defining simulation time
To set up the transient analysis
1
From Capture’s PSpice menu, choose New Simulation
Profile.
2
Enter a name for the new simulation profile.
3
Click OK.
4
In the Analysis Type list box on the Analysis tab, select
Time Domain (Transient).
5
In the Run to Time text box, type the duration of the
transient analysis.
6
Click OK.
Adjusting simulation parameters
Use the Options tab of the Simulation Settings dialog box to
adjust the simulation behavior of your circuit’s digital devices.
558
PSpice User's Guide
Product Version 10.5
Adjusting simulation parameters
To access the digital settings in the Options tab
1
From Capture’s PSpice menu, choose Edit Simulation
Profile.
2
Click the Options tab.
3
In the Category list box, select Gate-level simulation.
Each of the dialog box settings is described in the
following sections. For additional options, see Output
control options on page 573.
PSpice User's Guide
559
Chapter 14
Digital simulation
Product Version 10.5
Selecting propagation delays
All digital devices—including primitives and library models—
perform simulations using either minimum, typical, maximum
or worst-case (min/max) timing characteristics. You can set
the delay circuit-wide or on individual device instances.
Note: Propagation delay modeling is not available in PSpice
A/D Basics
Circuit-wide propagation delays
You can set these to minimum, typical, maximum or variable
within the min/max range for digital worst-case timing
simulation on the Options tab of the Simulation Settings dialog
box.
To specify the delay level circuit-wide
1
From Capture’s PSpice menu, choose Edit Simulation
Profile.
2
Click the Options tab.
3
In the Category list box, select Gate-level simulation.
Part instance propagation delays
You can set the propagation delay mode on an individual
device, thereby overriding the circuit-wide delay mode.
To override the circuit-wide default on an individual part
1
Set the part’s MNTYMXDLY property from 1 to 4 where
1
2
3
4
560
=
=
=
=
minimum
typical
maximum
worst-case (min/max)
PSpice User's Guide
Product Version 10.5
Adjusting simulation parameters
By default, MNTYMXDLY is set to 0, which tells
PSpice A/D to use the circuit-wide value defined in the
Options tab.
PSpice User's Guide
561
Chapter 14
Digital simulation
Product Version 10.5
Initializing flip-flops
To initialize all flip-flops and latches
Select one of the three Flip-flop Initialization choices on the
Options tab:
❑
If set to X, all flip-flops and latches produce an X
(unknown state) until explicitly set or cleared, or until
a known state is clocked in.
Note: The X initialization is the safest setting, since
many devices do not power up to a known state.
However, the 0 and 1 settings are useful in situations
where the initial state of the flip-flop is unimportant to
the function of the circuit, such as a toggle flip-flop in
a frequency divider.
❑
If set to 0, all such devices are cleared.
❑
If set to 1, all such devices are preset.
Refer to the online PSpice Reference Guide for more
information about flip-flops and latches.
Starting the simulation
To start the simulation
From the PSpice menu, choose Run.
After PSpice A/D completes the simulation, the graphical
waveform analyzer starts automatically.
562
PSpice User's Guide
Product Version 10.5
Starting the simulation
Analyzing results
PSpice A/D includes a graphical waveform analyzer for
simulation results. In effect, the waveform viewer in
PSpice A/D is a software oscilloscope. Running PSpice A/D
corresponds to building or changing a breadboard, and the
waveform viewer corresponds to looking at the breadboard
with an oscilloscope. You can observe and interactively
manipulate the waveform data produced by circuit simulation.
For a full discussion of how the waveform viewer is used to
analyze results, see Chapter 17, “Analyzing waveforms.”
For mixed analog/digital simulations, the waveform analyzer
can display analog and digital waveforms simultaneously with
a common time base.
PSpice A/D generates two forms of output: the simulation
output file and the waveform data file. The calculations and
results reported in the simulation output file are like an audit
trail of the simulation. However, the graphical analysis of
information stored in the data file is a more informative and
flexible method for evaluating simulation results.
To display waveforms
PSpice User's Guide
1
From the Trace menu, choose Add Trace.
2
Select traces for display:
563
Chapter 14
Digital simulation
Product Version 10.5
❑
In the Simulation Output Variables list, click any
waveforms you want to display. Each appears in the
Trace Expressions box at the bottom.
❑
Construct expressions by selecting operators,
functions and/or macros from the Functions or
Macros list, and output variables in the Simulation
Output Variables list.
❑
You can also type trace expressions directly into the
Trace Expression text box. A typical set of entries
might be:
IN1 IN2 Q1 Q2
Note: Use spaces or commas to separate the output
variables you place in the Trace Expressions list.
3
Click OK.
Waveforms for the selected output variables appear.
For detailed information on how to add digital traces, see
Digital trace expressions on page 703.
Adding digital signals to a plot
When defining digital trace expressions, you can include any
combination of digital signals, buses, signal constants, bus
constants, digital operators, macros and the Time sweep
variable.
The following rules apply:
■
An arithmetic or logical operation between two bus
operands results in a bus value that is wide enough to
contain the result.
■
An arithmetic or logical operation between a bus operand
and a signal operand results in a bus value.
The syntax for expressing a digital output variable or
expression is:
digital_output_variable [;display_name ]
or
564
PSpice User's Guide
Product Version 10.5
Starting the simulation
digital_expression [;display_name ]
Table 14-9
This placeholder...
Means this...
digital_output_
variable
output variable from the
Simulation Output Variable list
(Digital check box selected)
digital_expression
expression using digital output
variables and operators
display_name
(optional)
text string (name) to label the
signal on the plot, instead of
using the default output
variable notation
To add a digital trace expression
1
In the Add Traces dialog box, make sure you select the
Digital check box.
2
Do one of the following:
3
❑
In the Simulation Output Variables list, click the
signal you want to display.
❑
In the Trace Expression text box, create a digital
expression by either typing the expression, or by
selecting digital output variables from the Simulation
Output Variables list and digital operators from the
Digital Operators and Functions list.
If you want to label a signal with a name that is different
from the output variable:
a. Click in the Trace Expression text box after the last
character in the signal name.
b. Type ;display_name where display_name is the
name of the label.
Example: U2:Y;OUT1
where U2:Y is the output variable. On the plot, the signal
is labeled OUT1.
PSpice User's Guide
565
Chapter 14
Digital simulation
Product Version 10.5
Adding buses to a waveform plot
You can evaluate and display a set of up to 32 signals as a bus
even if the selected signals were not originally a bus.
This is done by following the same procedure already given for
adding digital signals to the plot. However, when adding a bus,
be sure to enclose the list of signals in braces: { }.
{ Q3 Q2 Q1 Q2 }
The complete syntax is as follows:
{signal_list}[;[display_name][;radix]]
or
{bus_prefix[msb:lsb]}[;[display_name][;radix]]
Table 14-10
This placeholder...
Means this...
signal_list
comma- or space-separated list of
up to 32 digital node names, in
sequence from high order to low
order
bus_prefix[msb:lsb]
alternate way to express up to 32
signals in the bus
display_name
(optional)
text string (name) to label the bus
on the plot, instead of using the
default output variable notation
Note: To change the radix without
changing the display name,
be sure to include two
consecutive semicolons.
Example:
{A3,A2,A1,A0};;radix
radix
(optional)
566
numbering system in which to
display bus values
PSpice User's Guide
Product Version 10.5
Starting the simulation
Valid entries for radix are shown in the following table.
Table 14-11
For this numbering system... Use this
notation...
Binary (base 2)
B
Decimal (base 10)
D
Hexadecimal (base 16)
H or X
Octal (base 8)
O (the letter)
To add a bus expression
1
In the Add Traces dialog box, in the Functions and Macros
list, choose Digital Operators and Constants.
2
Click the { } entry.
3
In the Simulation Output Variables list, select the signals
in high-order to low-order sequence.
4
If you want to label the bus with a name that is different
from the default:
a. Click in the Trace Expression text box after the last
character in the bus name.
b. Type ;display_name where display_name is the
name of the label.
5
If you want to set the radix to something different from the
default:
a. Click in the Trace Expression text box after the last
character in the expression.
b. Type one of the following where radix is a value from
Table 14-11:
❍
PSpice User's Guide
If you specified a display_name, then type
;radix.
567
Chapter 14
Digital simulation
Product Version 10.5
❍
If you did not specify a display_name, then
type ;;radix (two semicolons preceding the
radix value).
Examples:
568
■
{Q2,Q1,Q0};A;O specifies a 3-bit bus whose most
significant bit is Q2. PSpice A/D labels the plot A, and
values appear in octal notation.
■
{a3,a2,a1,a0};;d specifies a 4-bit bus. On the plot,
values appear in decimal notation. Since no display name
is specified, PSpice A/D uses the signal list as a label.
■
{a[3:0]} is equivalent to {a3,a2,a1,a0}
PSpice User's Guide
Product Version 10.5
Starting the simulation
Tracking timing violations and hazards
When there are problems with your design, such as
setup/hold violations, pulse-width violations, or worst-case
timing hazards, PSpice A/D saves messages to the simulation
output file or data file. You can select messages and have the
associated waveforms and detailed message text
automatically appear. The messaging feature is discussed
further in Tracking digital simulation messages on page 687 of
Chapter 17, “Analyzing waveforms.”
PSpice A/D can also detect persistent hazards that may have
a potential effect on a primary circuit output or on the internal
state of the design.
Note: This feature is not available in PSpice A/D Basics
Persistent hazards
Digital problems are usually either timing violations or timing
hazards. Timing violations include SETUP, HOLD and
minimum pulse WIDTH violations of component
specifications. This type of violation may produce a change in
the state behavior of the design, and potentially in the answer.
However, the effects of many of these errors are short-lived
and do not influence the final circuit results.
For example, consider an asynchronous data change on the
input to flip-flop FF1 in Figure 14-2 below. The data change is
too close to the clock edge e1, resulting in a SETUP violation.
In a hardware implementation, the output of FF1 may or may
not change. However, some designs are not sensitive to this
individual missed data because the next clock edge (e2 in this
example) latches the data. The designer must judge the
PSpice User's Guide
569
Chapter 14
Digital simulation
Product Version 10.5
significance of timing errors, accounting for the overall
behavior of the design.
O1
S
D Q
D Q
FF1
FF2
C ~Q
C ~Q
...
O2
...
O3
e1 e2
Figure 14-2 Circuit with a timing error.
Timing hazards are most easily identified by simulating a
design in worst-case timing mode, usually close to its critical
timing limits. Under such conditions, PSpice A/D reports
conditions such as AMBIGUITY CONVERGENCE hazards.
Again, these may or may not pose a problem to the operation
of the design.
However, there are identifiable cases that cause major
problems. An example of a major problem is shown in
Figure 14-3 below. Due to the simultaneous arrival of two
timing ambiguities (having unrelated origins, therefore nothing
in common) at the inputs to gate G1, PSpice A/D reports the
occurrence as an AMBIGUITY CONVERGENCE hazard. This
means that the output of G1 may glitch.
0
Figure 14-3 Circuit with a timing ambiguity
Note that the output fans out to two devices, G2 and L1. The
effects of a glitch on G1 in this case do not reach the circuit
570
PSpice User's Guide
Product Version 10.5
Starting the simulation
output P1, because that path is not sensitized (since the other
input to G2 is held LO and thus blocks the symptom).
However, because G1’s output is also used to clock latch L1,
the effects of a glitch could result in visibly incorrect behavior
on output P2. This is an example of a persistent hazard.
A persistent hazard is a timing violation or hazard that has a
potential effect on a primary (external) circuit output or on the
internal state (stored state or memory elements) of the design.
For the design to be considered reliable, you must correct
such timing hazards.
PSpice A/D fully distinguishes between state uncertainty and
time uncertainty. When a hazard occurs, PSpice A/D
propagates hazard origin information along with the machine
state through all digital devices. When a hazard propagates to
a state-storage device primitive (JKFF, DFF, SRFF, DLTCH,
RAM), PSpice A/D reports a PERSISTENT HAZARD.
Simulation condition messages
PSpice A/D produces warning messages in various
situations, such as those that originate from the digital
CONSTRAINT devices monitoring timing relationships of
digital nodes. These messages are directed to the simulation
output file and/or to the waveform data file. Options are
available for controlling where and how many of these
messages are generated, as summarized later in this section.
Table 14-12 below summarizes the simulation message types,
with a brief description of their meaning. Currently, the
messages supported are specific to digital device timing
violations and hazards.
Table 14-12 Simulation condition messages—timing violations
Message type
Severity level
Meaning
SETUP
WARNING
Minimum time required for a data signal to be stable
prior to the assertion of a clock was not met.
HOLD
WARNING
Minimum time required for a data signal to be stable
after the assertion of a clock was not met.
PSpice User's Guide
571
Chapter 14
Digital simulation
Product Version 10.5
Table 14-12 Simulation condition messages—timing violations
Message type
Severity level
Meaning
RELEASE
WARNING
Minimum time required for a signal that has gone
inactive (usually a control such as CLEAR) to remain
inactive before the asserting clock edge was not met.
WIDTH
WARNING
Minimum pulse width specification for a signal was not
satisfied; that is, a pulse that was too narrow was
observed on the node.
FREQUENCY
WARNING
Minimum or maximum frequency specification for a
signal was not satisfied. Minimum frequency violations
indicate that the period of the measured signal is too
long, while maximum frequency violations describe
signals changing too rapidly.
GENERAL
INFO
Boolean expression described within the GENERAL
constraint checker was evaluated and produced a true
result.
Table 14-13 Simulation condition messages—hazards
Message type
Severity level
Meaning
AMBIGUITY
CONVERGENCE
WARNING
Convergence of conflicting rising and falling states
(timing ambiguities) arrived at the inputs of a primitive
and produced a pulse (glitch) on the output. See
Chapter 16, “Digital worst-case timing analysis” for
more information.
CUMULATIVE
AMBIGUITY
WARNING
Signal ambiguities are additive, increased by
propagation through each level of logic in the circuit.
The ambiguities associated with both edges of a
pulse increased to the point where they overlapped,
which PSpice A/D reports as a cumulative ambiguity
hazard. See Chapter 16, “Digital worst-case timing
analysis” for more information.
572
PSpice User's Guide
Product Version 10.5
Starting the simulation
Table 14-13 Simulation condition messages—hazards
Message type
Severity level
Meaning
SUPPRESSED
GLITCH
WARNING
Pulse applied to the input of a primitive that is shorter
than the active propagation delay was ignored by
PSpice A/D; significance depends on the nature of
the circuit. There might be a problem either with the
stimulus, or with the path delay configuration of the
circuit. See Chapter 16, “Digital worst-case timing
analysis” for more information.
NET-STATE
CONFLICT
WARNING
Two or more outputs attempted to drive a net to
different states, which PSpice A/D reports as an X
(unknown) state. This usually results from improper
selection of a bus driver’s enable inputs.
ZERO-DELAYOSCILLATION
FATAL
Output of a primitive changed more than 50 times
within a single digital time step. PSpice A/D aborted
the run.
DIGITAL INPUT
VOLTAGE
SERIOUS
Voltage on a digital pin was out of range, which
means PSpice A/D used the state with a voltage
range closest to the input voltage and continued the
simulation.
PERSISTENT
HAZARD
SERIOUS
Effects of any of the aforementioned logic hazards
were able to propagate to either an external port or to
any storage device in the circuit. See Persistent
hazards on page 569 for more information.
Output control options
Four control options are available for managing the generation
of simulation condition messages. These are described in
Table 14-14.
To access these commands, select the Options tab in the
Simulation Settings dialog box. You can set NOOUTMSG and
NOPRBMSG by selecting the Output file Category. You can
set DIGERRDEFAULT and DIGERRLIMIT by selecting the
PSpice User's Guide
573
Chapter 14
Digital simulation
Product Version 10.5
Gate-level simulation Category and clicking Advanced
Options.
Table 14-14 Simulation message output control options
This option...
Means this...
NOOUTMSG
Suppresses the recording of
simulation condition messages in
the simulation output file.
NOPRBMSG
Suppresses the recording of
simulation condition messages in
the waveform data file.
DIGERRDEFAULT=<n> Establishes a default limit, n, to
the number of condition messages
that may be generated by any
digital device that has a constraint
checker primitive without a local
default. If global or local defaults
are unspecified, there is no limit.
DIGERRLIMIT=<n>
Establishes an upper limit, n, for
the total number of condition
messages that may be generated
by any digital device. If this limit is
exceeded, PSpice A/D aborts the
run. By default, the total number of
messages is 20.
Severity levels
PSpice A/D assigns one of four severity levels to the
messages:
■
FATAL
■
SERIOUS
■
WARNING
■
INFO (informational)
FATAL conditions cause PSpice A/D to cancel the simulation.
Under all other severity levels, PSpice A/D continues to run.
574
PSpice User's Guide
Product Version 10.5
Starting the simulation
The severity levels are used to filter the classes of messages
that are displayed when loading a data file.
PSpice User's Guide
575
Chapter 14
576
Digital simulation
Product Version 10.5
PSpice User's Guide
Mixed analog/digital simulation
15
Chapter overview
This chapter describes how PSpice A/D runs mixed
analog/digital simulations and includes the following sections:
■
Interconnecting analog and digital parts on page 578
■
Interface subcircuit selection by PSpice on page 579
■
Specifying digital power supplies on page 583
■
Interface generation and node names on page 589
Note: This entire chapter describes features that are not
included in PSpice.
PSpice User's Guide
577
Chapter 15
Mixed analog/digital simulation
Product Version 10.5
Interconnecting analog and digital parts
Prior to simulation, netlisting translates the part instances and
nets defined in your schematic into parts connected by nodes.
The standard simulation netlist contains a flat view of the
circuit. You can also create hierarchical netlists. PSpice A/D
extracts the definitions for all parts modeled as subcircuits,
viewing parts as a collection of primitive parts and node
connections.
The digital primitives that make up a digital part determine the
way that PSpice A/D processes an analog/digital interface to
that part. Specifically, the I/O model for each digital primitive
connected at the interface gives PSpice A/D the necessary
information.
PSpice A/D recognizes three types of nodes: analog nodes,
digital nodes, and interface nodes. The node type is
determined by the types of parts connected to it. If all of the
parts connected to a node are analog, then it is an analog
node. If all of the parts are digital, then it is a digital node. If
there is a combination of analog and digital parts, then it is an
interface node.
PSpice A/D automatically breaks interface nodes into one
purely analog and one or more digital nodes by inserting one
or more analog/digital interface subcircuits.
PSpice A/D also automatically connects a power supply to the
interface subcircuit to complete the generation of the interface.
To view simulation results at an analog/digital interface in your
schematic using the graphical waveform analyzer:
578
■
Place a marker on the appropriate interface net. The
additional nodes created by PSpice A/D remain
transparent.
■
View results in PSpice A/D by selecting traces from the
output variable list (from the Trace menu, choose Add
Trace). If you use this approach, note the names
PSpice A/D generates for the new nodes. To find out
more, see Interface generation and node names on
page 589.
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
Interface subcircuit selection by PSpice
Analog-to-digital (AtoD) and digital-to-analog (DtoA) interface
subcircuits handle the translation between analog voltages/
impedances and digital states, or vice-versa. The main
component of an interface subcircuit is either a PSpice N part
(digital input: digital-to-analog) or a PSpice O (that’s the letter
O, not the numeral zero) part (digital output: analog-to-digital).
PSpice N and O parts are neatly packaged into interface
subcircuits in the model library. The standard model library
shipped with your software installation includes interface
subcircuits for each of the supported logic families: TTL,
CD4000 series CMOS and high-speed CMOS (HC/HCT),
ECL 10K, and ECL 100K. This frees you from ever having to
define them yourself when using parts in the standard library.
If you are creating custom digital parts in technologies other
than those provided in the standard model library, you may
need to create your own interface subcircuits.
Note: To search for particular parts in the standard PSpice
libraries, see the online PSpice Library List.
Every digital primitive comprising the subcircuit description of
a digital part has an I/O model describing its loading and
driving characteristics. The name of the interface subcircuit
actually inserted by PSpice A/D is specified by the I/O model
of the digital primitive at the interface. The I/O model has
parameters for up to four analog-to-digital (AtoD) and four
digital-to-analog (DtoA) subcircuit names.
You can choose among four interface levels of subcircuit
models, depending on the simulation accuracy you need. In
some cases you may need more accurate simulations of the
input/output stages of a digital part, while in other cases, a
simpler, smaller model is enough.
Digital parts provided in the standard libraries only use
interface levels 1 and 2. With the exception of the HC/HCT
series (described below), levels 3 and 4 reference the same
subcircuits as levels 1 and 2. Table 15 below summarizes the
four interface levels.
PSpice User's Guide
579
Chapter 15
Mixed analog/digital simulation
Product Version 10.5
The difference between levels 1 and 2 only occurs in the AtoD
interfaces, described below. In all cases, the level 1 DtoA
interface is the same as the level 2 DtoA interface, except that
the level 2 DtoA interface does not generate intermediate R,
F, and X levels.
Table 15-1 Interface subcircuit models
Level
Subcircuits
Definition
1
AtoD1/DtoA1
AtoD generates intermediate R, F,
and X levels
2
AtoD2/DtoA2
AtoD does not generate
intermediate R, F, and X levels
3
AtoD3/DtoA3
(same as level 1)
4
AtoD4/DtoA4
(same as level 2)
The OrCAD libraries provide two different DtoA models in the
HC/HCT series: the simple model and the elaborate model.
You can use the simple model by specifying level 1 or 2, the
elaborate model by specifying level 3 or 4. The elaborate
model is noticeably slower than the simple model, so you
should only use it if you are using a power supply level other
than 5.0 volts.
The HC/HCT level 1 and 2 DtoA models produce accurate I-V
curves given a fixed power supply of 5.0 volts and a
temperature of 25°C. The level 3 and 4 DtoA models produce
accurate I-V curves over the acceptable range of power
supply voltages (2-6 volts), and they include temperature
derating.
Level 1 interface
The level 1 AtoD interface generates intermediate logic levels
(R, F, X) between the voltage ranges VILMAX and VIHMIN
(specific voltages depend on the technology you are using). A
steadily rising voltage on the input of the AtoD will transition
from 0 to R at VILMAX and from R to 1 at VIHMIN. The F level
is output for steadily falling voltages in a similar manner. The
580
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
X level is produced if the input voltage starts in the threshold
region or doubles back into a previously crossed threshold.
Level 1 (the default) strictly maps logic levels onto the
changing input voltage. The exact switching voltage is
assumed to be anywhere between VILMAX and VIHMIN due
to temperature or power supply variations. Thus, it provides
more accurate, less optimistic results.
This behavior may not be appropriate when the input rise and
fall times are long, or when the input voltage never leaves the
threshold region. If this is the case, you may want to use the
level 2 interface.
Level 2 interface
The level 2 AtoD interface transitions directly from 0 to 1 and
1 to 0 without passing through intermediate R, F, or X levels.
An exact switching voltage is assumed (again, the specific
voltage depends on the technology you are using). It provides
a more optimistic, and therefore less accurate, response than
level 1. Level 2’s behavior is appropriate when the input
voltage oscillates around the threshold voltage.
Note: You can avoid simulations that get bogged down with
the greater detail of R, F, and X states around these
oscillations. You may want to specify level 2 on only
those parts for which this behavior is critical to a
successful simulation. This is described in Setting the
default A/D interface below.
PSpice User's Guide
581
Chapter 15
Mixed analog/digital simulation
Product Version 10.5
Setting the default A/D interface
For mixed-signal simulation, you can select the AtoD and
DtoA interface level circuit-wide and on individual part
instances.
■
To select the default interface level circuit-wide, select
one of the four Default A/D interfaces in the Simulation
Settings dialog box by selecting the Gate-level simulation
category under the Options tab. Part instances with the
IO_LEVEL property set to 0 use this value.
■
You can override the circuit-wide default on an individual
part by specifying an IO_LEVEL property from 1 to 4,
where:
1:
AtoD1 and DtoA1 (default)
2:
AtoD2 and DtoA2
3:
AtoD3 and DtoA3
4:
AtoD4 and DtoA4
For example, you can tell the simulator to use the level 2
interface subcircuits for a 7400 part by setting the IO_LEVEL
property to 2. All other part instances continue to use the
circuit-wide setting. By default, IO_LEVEL is set to 0, which
tells the simulator to use the circuit-wide level defined in the
Gate-level simulation category in the Simulation Settings
dialog box.
582
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
Specifying digital power supplies
Digital power supplies are used to power interface subcircuits
that are automatically created by PSpice A/D when simulating
analog/digital interfaces. They are specified as follows:
■
PSpice A/D can instantiate them automatically.
■
You can create your own digital power supplies and place
them in your design.
When using parts from the standard libraries in your design,
you can usually have PSpice A/D automatically create the
necessary digital power supply. If you use custom digital parts
created in technologies other than those provided in the
standard model library, you may need to create your own
digital power supplies.
Because digital power supplies are used only by analog/digital
interface subcircuits, digital power supplies are not needed for
digital-only designs. We recommend avoiding placing a power
supply to a digital-only design because it may increase
simulation time and memory usage.
Default power supply selection by PSpice A/D
When PSpice A/D encounters an analog/digital interface, it
creates the appropriate interface subcircuit and power supply
according to the I/O model referenced by the digital part. The
I/O model is specific to the digital part’s logic family. The power
supply provides reference or drive voltage for the analog side
of the interface.
By default, PSpice A/D inserts one power supply subcircuit for
every logic family in which a digital primitive is involved with an
analog/digital interface. These power supply subcircuits
create the digital power and ground nodes that are the
defaults for all parts in that family. If multiple digital primitives
from the same logic family are involved with analog/digital
interfaces, one instance of the power supply subcircuit is
created with all primitives connected to the power supply
nodes.
PSpice User's Guide
583
Chapter 15
Mixed analog/digital simulation
Product Version 10.5
Table 15-2 summarizes the default node names and values.
For instance, TTL power supplies have a default value of 5.0
volts at analog/digital interfaces.
Table 15-2 Default digital power/ground pin connections
Logic
family
Digital power/
ground pin properties
Default digital power/ground
nodes
TTL
PSPICEDEFAULTNET
(PWR)
$G_DPWR (5.0 volts)
$G_DGND (0 volts)
PSPICEDEFAULTNET
(GND)
CD4000 PSPICEDEFAULTNET
(VDD)
$G_CD4000_VDD (5 volts)
$G_CD4000_VSS (0 volts)
PSPICEDEFAULTNET (VSS)
ECL 10K PSPICEDEFAULTNET (VEE) $G_ECL_10K_VEE (-5.2 volts)
$G_ECL_10K_VCC1 (0 volts)
PSPICEDEFAULTNET
$G_ECL_10K_VCC2 (0 volts)
(VCC1)
PSPICEDEFAULTNET
(VCC2)
ECL
100K
PSPICEDEFAULTNET (VEE) $G_ECL_100K_VEE (-4.5 volts)
$G_ECL_100K_VCC1 (0 volts)
PSPICEDEFAULTNET
$G_ECL_100K_VCC2 (0 volts)
(VCC1)
PSPICEDEFAULTNET
(VCC2)
The PSPICEDEFAULTNET pin properties have the same
default values as the digital power and ground nodes created
by the default power supply. These node assignments are
passed from the part instance to the digital primitives
describing its behavior, connecting any digital primitive
affected by an analog connection to the correct power supply.
The default I/O models and power supply subcircuits are
found in DIG_IO.LIB. The four default power supplies provided
in the model library are DIGIFPWR (TTL), CD4000_PWR
(CD4000 series CMOS), ECL_10K_PWR (ECL 10K), and
ECL_100K_PWR (ECL 100K).
584
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
Creating custom digital power supplies
Each digital part model has optional digital power and ground
nodes that you can use to specify custom power supplies. To
do this, use one of the digital power supplies listed in Table
15-3 below in your design and redefine the digital power
supply nodes.
Table 15-3 Digital power supply parts in SPECIAL.OLB
Part type
(PSpice A/D X model)
Part name
CD4000 power supply
CD4000_PWR
TTL power supply
DIGIFPWR
ECL 10K power supply
ECL_10K_PWR
ECL 100K power supply
ECL_100K_PWR
When creating custom power supplies, you can refer to the
power supply definitions in DIG_IO.LIB for examples of power
supply subcircuit definitions. The properties relevant to
creating custom power supplies are shown in Table 15-4.
Table 15-4 Digital power supply properties
Part name
Property
Description
CD4000_PWR
VOLTAGE
CD4000 series CMOS power
supply voltage
PSPICEDEFAULTNET
CD4000 series CMOS hidden
power supply pins for VDD and
VSS
VOLTAGE
TTL power supply voltage
PSPICEDEFAULTNET
TTL hidden power (PWR) and
ground (GND) pins
DIGIFPWR
PSpice User's Guide
585
Chapter 15
Mixed analog/digital simulation
Product Version 10.5
Part name
Property
Description
ECL_10K_PWR
ECL_100K_PWR
VEE
VCC1
VCC2
ECL power supply voltages
PSPICEDEFAULTNET
ECL hidden power supply pins for
VEE, VCC1 and VCC2
To create a custom digital power supply
Note: This procedure applies to all logic families.
1
Place the appropriate power supply part listed in Table
15-3 in your design (by logic family).
2
Rename the power supply power and ground pins
(PSPICEDEFAULTNET properties).
3
Reset the power supply power and ground voltages as
required.
4
For any digital part instance that uses the power supply,
set its appropriate PSPICEDEFAULTNET pin properties
to the power and ground pins created by the secondary
power supply.
Overriding CD4000 power supply voltage throughout a design
Designs using CD4000 parts often require power supply
voltages other than the default 5.0 volts supplied by the
standard CD4000_PWR power supply part. If needed, you
can override the power supply voltage for all CD4000 parts in
a design.
The default power supply nodes used by CD4000 parts are
named $G_CD4000_VDD and $G_CD4000_VSS as created
by the power supply subcircuit CD4000_PWR. This supply
defaults to 5.0 volts. You can override the voltage across these
two nodes by defining values for the parameters named
CD4000_VDD and CD4000_VSS that are referenced by the
CD4000_PWR subcircuit definition.
586
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
To change the CD4000_PWR power supply to 12 volts,
referenced to ground:
1
Place an instance of the PARAM pseudopart from
SPECIAL.OLB.
2
Create a new PARAM property as follows:
CD4000_VDD = 12.0V
DC4000_VSS is left at its default of 0 volts.
If the reference voltage also needs to be reset, the same
method can be used to define the CD4000_VSS parameter by
setting this property of the same PARAM instance. For
example, if you want the supplies to go between -5 volts and
+5 volts (a difference of 10 volts), set CD4000_VSS to -5V and
CD4000_VDD to +10V; as a result, CD4000_VDD is 10 volts
above CD4000_VSS, or +5 volts.
Creating a secondary CD4000, TTL, or ECL power supply
Designs using CD4000, TTL, or ECL parts may require power
supply voltages in addition to the default 5.0 volts supplied by
the standard CD4000_PWR power supply part.
To create a secondary power supply for any one of the
CD4000, TTL, or ECL technologies, you must place the
appropriate power supply part and create user-defined nodes
with a new voltage value.
Note: Designs with TTL and ECL parts rarely require
secondary power supplies. If needed, however, you
can use this procedure to add a secondary power
supply for TTL and ECL parts.
To create and use a secondary CD4000 power supply with
nodes MY_VDD and MY_VSS and a voltage of 3.5 volts:
1
Place the CD4000_PWR power supply and modify the
appropriate pin properties as follows:
VOLTAGE = 3.5V
PSPICEDEFAULTNET = MY_VDD
PSPICEDEFAULTNET = MY_VSS
PSpice User's Guide
587
Chapter 15
Mixed analog/digital simulation
2
Product Version 10.5
Select a CD4000 part in the schematic to which the new
power supply should apply, then change the appropriate
pin properties as follows:
PSPICEDEFAULTNET = MY_VDD
PSPICEDEFAULTNET = MY_VSS
588
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
Interface generation and node names
The majority of the interface generation process involves
PSpice A/D determining whether analog and digital primitives
are connected, and if so, inserting an interface subcircuit for
each digital connection. This turns the interface node into a
purely analog node, which now connects to the analog
terminal of the interface subcircuit. To complete the original
connection, PSpice A/D creates a new digital node between
the digital terminal of the interface subcircuit and the digital
primitive.
Because PSpice A/D must create new digital nodes, it must
give them unique names. These node names are used in the
output variables in the list of viewable traces when you choose
Add Trace from the Trace menu. Name generation follows
these rules:
■
The analog node retains the name of the original interface
node—either the labeled wire name in the design, or the
node name automatically generated for an unlabeled
wire.
■
Each new digital node name consists of the labeled wire
name in the design or the node name automatically
generated for an unlabeled wire, appended with $AtoD or
$DtoA. If the node is attached to more than one digital
part, the second digital node is appended with $AtoD2 or
$DtoA2, and so on.
Figure 15-1 below shows a fragment of a mixed analog/digital
circuit before and after the interface subcircuits have been
added. The wires labeled 1 and 2 in the schematic
representation are the interface nets connecting analog and
digital parts. These translate to interface nodes, which are
PSpice User's Guide
589
Chapter 15
Mixed analog/digital simulation
Product Version 10.5
processed by PSpice A/D to create the circuit fragment shown
in the PSpice A/D representation.
schematic representation
PSpice A/D representation
Figure 15-1 Mixed analog/digital circuit before
and after interface generation.
After interface generation, node 1 is a purely analog node,
connecting the resistor, transistor, and the analog inputs of
both AtoD subcircuits. Node 2 is also a purely analog node,
connecting the resistor and the analog output of the DtoA
interface. You can see that PSpice A/D inserted two new
digital nodes, 1$AtoD and 1$AtoD2, which connect the
outputs of the AtoD interfaces to the inverter inputs. It also
created one digital node, 2$DtoA, to connect the output of U1
to the digital input of the DtoA interface.
The interface subcircuits PSpice A/D automatically generates
are listed in the simulation output file under the section named
Generated AtoD and DtoA Interfaces. For the example in
Figure 15-1, this section would appear in the simulation output
file as shown in Figure 15-2 below.
590
PSpice User's Guide
Product Version 10.5
Interface subcircuit selection by PSpice
**** Generated AtoD and DtoA Interfaces ****
*
* Analog/Digital interface for node 1
*
* Moving X1.U1:.A from analog node 1 to new digital node * 1$AtoD
X$1_AtoD1 1 1$AtoD $G_DPWR $G_DGND AtoD_STD
+ PARAMS: CAPACITANCE= 0
* Moving X2.U1:.A from analog node 1 to new digital node * 1$AtoD2
X$1_AtoD2 1 1$AtoD $G_DPWR $G_DGND AtoD_STD
+ PARAMS: CAPACITANCE= 0
*
* Analog/Digital interface for node 2
*
** Moving X1.U1.Y from analog node 2 to new digital node * 2$DtoA
X$2_DtoA1 2$DtoA 2 $G_DPWR $G_DGND DtoA_STD
+ PARAMS: DRVL=0 DRVH=0 CAPACITANCE=0
*
* Analog/Digital interface power supply subcircuit
*
X$DIGIFPWR 0 DIGIFPWR
.END ;(end of AtoD and DtoA interfaces)
Figure 15-2 Simulation output for mixed analog/digital
circuit.
The lines that begin with “Moving…from analog node” indicate
the new digital node names that were generated. Below each
of these are the interface subcircuit calls inserted by
PSpice A/D.
In this example, the subcircuits named AtoD_STD and
DtoA_STD are obtained from the I/O model that is referenced
by the inverter primitive inside the subcircuit describing the
7404 part. The CAPACITANCE, DRVL (low-level driving
resistance), and DRVH (high-level driving resistance)
subcircuit parameter values come from the same I/O model.
After the interface subcircuit calls, PSpice A/D inserts one or
more interface power supply subcircuits. The subcircuit name
is specified in the I/O model for the digital primitive at the
interface. In this example, PSpice A/D inserted DIGIFPWR,
which is the power supply subcircuit used by all TTL models in
the model library. DIGIFPWR creates the global nodes
$G_DPWR and $G_DGND, which are the default nodes used
by each TTL part.
PSpice User's Guide
591
Chapter 15
592
Mixed analog/digital simulation
Product Version 10.5
PSpice User's Guide
Digital worst-case timing
analysis
16
This chapter deals with worst-case timing analysis and
includes the following sections:
■
Digital worst-case timing on page 594
■
Starting digital worst-case timing analysis on page 596
■
Simulator representation of timing ambiguity on page 596
■
Propagation of timing ambiguity on page 598
■
Identification of timing hazards on page 599
■
Convergence hazard on page 599
■
Critical hazard on page 600
■
Cumulative ambiguity hazard on page 601
■
Reconvergence hazard on page 603
■
Glitch suppression due to inertial delay on page 605
■
Methodology on page 606
Note: This entire chapter describes features that are not
included in PSpice.
PSpice User's Guide
593
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
Digital worst-case timing
Manufacturers of electronic components generally specify
component parameters (such as propagation delays in the
case of logic devices) as having tolerances. These are
expressed as either an operating range, or as a spread around
a typical operating point. The designer then has some
indication of how much deviation from typical one might
expect for any of these particular component delay values.
Realizing that any two (or more) instances of a particular type
of component may have propagation delay values anywhere
within the published range, designers are faced with the
problem of ensuring that their products are fully functional
when they are built with combinations of components having
delay specifications that fall (perhaps randomly) anywhere
within this range.
Historically, this has been done by making simulation runs
using minimum (MIN), typical (TYP), and maximum (MAX)
delays, and verifying that the product design is functional at
these extremes. But, while this is useful to some extent, it
does not uncover circuit design problems that occur only with
certain combinations of slow and fast parts. True digital
worst-case simulation, as provided by PSpice A/D, does just
that.
Other tools called timing verifiers are sometimes used in the
design process to identify problems that are indigenous to
circuit definition. They yield analyses that are inherently
pattern-independent and often pessimistic in that they tend to
find more problems than will truly exist. In fact, they do not
consider the actual usage of the circuit under an applied
stimulus.
PSpice A/D does not provide this type of static timing
verification. Digital worst-case timing simulation, as provided
by PSpice A/D, is a pattern-dependent mechanism that allows
a designer to locate timing problems subject to the constraints
of a specific applied stimulus.
Note: Digital worst-case timing analysis is not available
PSpice A/D Basics.
594
PSpice User's Guide
Product Version 10.5
Digital worst-case timing
Digital worst-case analysis compared to analog worst-case analysis
Digital worst-case timing simulation is different from analog
worst-case analysis in several ways. Analog worst-case
analysis is implemented as a sensitivity analysis for each
parameter which has a tolerance, followed by a projected
worst-case simulation with each parameter set to its minimum
or maximum value. This type of analysis is general since any
type of variation caused by any type of parameter tolerance
can be studied. But it is time consuming since a separate
simulation is required for each parameter. This does not
always produce true worst-case results, since the algorithm
assumes that the sensitivity is monotonic over the tolerance
range.
The techniques used for digital worst-case timing simulation
are not compatible with analog worst-case analysis. It is
therefore not possible to do combined analog/digital
worst-case analysis and simulation and get the correct results.
PSpice A/D allows digital worst-case simulation of
mixed-signal and all-digital circuits; any analog sections are
simulated with nominal values.
Systems containing embedded analog-within-digital sections
do not give accurate worst-case results; they may be
optimistic or pessimistic. This is because analog simulation
can not model a signal that will change voltage at an unknown
point within some time interval.
PSpice User's Guide
595
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
Starting digital worst-case timing analysis
To set up a digital worst-case timing analysis:
1
In the Simulation Settings dialog box, click the Options
tab.
See Setting up analyses on page 373 for a description of
the Simulation Settings dialog box.
2
Under Category, select Gate-level Simulation.
3
In the Timing Mode frame, check Worst-case (min/max)
4
In the Initialize all flip-flops drop-down list, select X.
5
Set the Default I/O level for A/D interfaces to 1.
6
Click OK.
7
Start the simulation as described in Starting a simulation
on page 385.
Simulator representation of timing ambiguity
PSpice A/D uses the five-valued state representation
{0,1,R,F,X}, where R and F represent rising and falling
transitions, respectively. Any R or F transitions can be thought
of as ambiguity regions. Although the starting and final states
are known (example: R is a 0 → 1 transition), the exact time of
the transition is not known, except to say that it occurs
somewhere within the ambiguity region. The ambiguity
region is the time interval between the earliest and the latest
time that a transition could occur.
Timing ambiguities propagate through digital devices via
whatever paths are sensitized to the specific transitions
involved. This is normal logic behavior. The delay values
(MIN, TYP, or MAX) skew the propagation of such signals by
whatever amount of propagation delay is associated with each
primitive instance.
When worst-case (MIN/MAX) timing operation is selected,
both the MIN and the MAX delay values are used to compute
596
PSpice User's Guide
Product Version 10.5
Simulator representation of timing ambiguity
the duration of the timing ambiguity result that represents a
primitive’s output change.
For example, consider the model of a BUF device in the
following figure.
U5 BUF $G_DPWR $G_DGND IN1 OUT1 ; BUFFER model
+ T_BUF IO_STD
.MODEL T_BUF UGATE (
; BUF timing model
+ TPLHMN=15ns TPLHTY=25ns TPLHMX=40ns
+ TPHLMN=12ns TPHLTY=20ns TPHLMX=35ns)
5
20
45
Figure 16-1 Timing ambiguity example one.
The application of the instantaneous 0-1 transition at 5nsec in
this example produces a corresponding output result. Given
the delay specifications in the timing model, the output edge
occurs at a MIN of 15nsec later and a MAX of 40nsec later.
The region of ambiguity for the output response is from 20 to
45nsec (from TPLHMN and TPLHMX values). Similar
calculations apply to a 1-0 transition at the input, using
TPHLMN and TPHLMX values.
PSpice User's Guide
597
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
Propagation of timing ambiguity
As signals propagate through the circuit, ambiguity is
contributed by each primitive having a nonzero MIN/MAX
delay spread. Consider the following example that uses the
delay values of the previous BUF model.
35
5
20
85
45
Figure 16-2 Timing ambiguity example two.
This accumulation of ambiguity may have adverse effects on
proper circuit operation. In the following example, consider
ambiguity on the data input to a flip-flop.
D
Q
C
Figure 16-3 Timing ambiguity example three.
The simulator must predict an X output, because it is not
known with any certainty when the data input actually made
the 0-1 transition. If the cumulative ambiguity present in the
data signal had been less, the 1 state would be latched up
correctly.
Figure 16-4 illustrates the case of unambiguous data change
(settled before the clock could transition) being latched up by
a clock signal with some ambiguity. The Q output will change,
but the time of its transition is a function of both the clock’s
ambiguity and that contributed by the flip-flop MIN/MAX
delays.
D
Q
C
Figure 16-4 Timing ambiguity example four.
598
PSpice User's Guide
Product Version 10.5
Identification of timing hazards
Identification of timing hazards
Timing hazard is the term applied to situations where the
response of a device cannot be properly predicted because of
uncertainty in the arrival times of signals applied to its inputs.
For example, Figure 16-5 below shows the following signal
transitions (0-1, 1-0) being applied to the AND gate.
Figure 16-5 Timing hazard example.
The state of the output does not (and should not) change,
since at no time do both input states qualify the gate, and the
arrival times of the transitions are known.
Convergence hazard
In cases where there are ambiguities associated with the
signal transitions 0-R-1 and 1-F-0—which have a certain
amount of overlap—it is no longer certain which of the
transitions happens first.
The output could pulse (0-1-0) at some point because the
input states may qualify the gate. On the other hand, the
output could remain stable at the 0 state. This is called a
convergence hazard because the reason for the glitch
occurrence is the convergence of the conflicting ambiguities at
two primitive inputs.
Gate primitives (including LOGICEXP primitives) that are
presented with simultaneous opposing R and F levels may
produce a pulse of the form 0-R-0 or 1-F-1.
For example, a two-input AND gate with the inputs shown in
Figure 16-6 below, produces the output shown.
Figure 16-6 Convergence hazard example.
PSpice User's Guide
599
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
This output (0-R-0) should be interpreted as a possible
single pulse, no longer than the duration of the R level.
Note: Other types of primitives, such as flip-flops, may
produce an X instead of an R-0 or F-1 in response to a
convergence hazard.
The actual device’s output may or may not change, depending
on the transition times of the inputs.
Critical hazard
It is important to note that the glitch predicted could propagate
through the circuit and may cause incorrect operation. If the
glitch from a timing hazard becomes latched up in an internal
state (such as flip-flop or ram), or if it causes an incorrect state
to be latched up, it is called a critical hazard because it
definitely causes incorrect operation.
Otherwise, the hazard may pose no problem. Figure 16-7
below shows the same case as above, driving the data input
to a latch.
D
Q
C
Figure 16-7 Critical hazard example.
As long as the glitch always occurs well before the leading
edge of the clock input, it will not cause a problem.
600
PSpice User's Guide
Product Version 10.5
Identification of timing hazards
Cumulative ambiguity hazard
In worst-case mode, simple signal propagation through the
network will result in a buildup of ambiguity along the paths
between synchronization points. See Glitch suppression due to
inertial delay on page 605. The cumulative ambiguity is
illustrated in Figure 16-8.
1
2
8
9
2
5
9
12
TPxxMN=1
TPxxMX=3
Figure 16-8 Cumulative ambiguity hazard example one.
The rising and falling transitions applied to the input of the
buffer have a 1nsec ambiguity. The delay specifications of the
buffer indicate that an additional 2nsec of ambiguity is added
to each edge as they propagate through the device. Notice
that the duration of the stable state 1 has diminished due to
the accumulation of ambiguity.
Figure 16-9 shows the effects of additional cumulative
ambiguity.
2
5
9
12
3
TPxxMN=1
TPxxMX=7
10
19
12
Figure 16-9 Cumulative ambiguity hazard example two.
The X result is predicted here because the ambiguity of the
rising edge propagating through the device has increased to
the point where it will overlap the later falling edge ambiguity.
Specifically, the rising edge should occur between 3nsec and
12nsec; but, the subsequent falling edge applied to the input
predicts that the output starts to fall at 10nsec. This situation
is called a cumulative ambiguity hazard.
Another cause of cumulative ambiguity hazard involves
circuits with asynchronous feedback. The simulation of such
circuits under worst-case timing constraints yields an overly
pessimistic result due to the unbounded accumulation of
PSpice User's Guide
601
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
ambiguity in the feedback path. A simple example of this effect
is shown in Figure 16-10.
OSC
OSC
Figure 16-10 Cumulative ambiguity hazard example
three.
Due to the accumulation of ambiguity in the loop, the output
signal will eventually become X, because the ambiguities of
the rising and falling edges overlap. However, in the hardware
implementation of this circuit, a continuous phase shift with
respect to absolute time is what will actually occur (assuming
normal deviations of the rise and fall delays from the nominal
values).
Note: If this signal were used to clock another circuit, it would
become the reference and the effects of the phase shift
could be ignored. You can do this by setting the NAND
gate’s model parameter, MNTYMXDLY=2 to utilize
typical delay values for that one gate only (all other
devices continue to operate in worst-case mode).
602
PSpice User's Guide
Product Version 10.5
Identification of timing hazards
Reconvergence hazard
PSpice A/D recognizes situations where signals having a
common origin reconverge on the inputs of a single device. In
Figure 16-11, the relative timing relationship between the two
paths (U2, U3) is important.
25
TPLHMN=10
TPLHMX=30
60
U2
D
t=0
15
30
U1
Q
U4
C
U3
TPLHMN=15
TPLHMX=30
TPLHMN=40
TPLHMX=60
55
90
Figure 16-11 Reconvergence hazard example one.
Given the delay values shown, it is impossible for the clock to
change before the data input, since the MAX delay of the U2
path is smaller than the MIN delay of the U3 path. In other
words, the overlap of the two ambiguity regions could not
actually occur.
PSpice A/D recognizes this type of situation and does not
produce the overly pessimistic result of latching an X state into
the Q-output of U4. This factors out the 15 nsec of common
ambiguity attributed to U1 from the U2 and U3 signals (see
Figure 16-12).
U2
25
45
U3
55
75
Figure 16-12 Reconvergence hazard example two.
The result in Figure 16-12 does not represent what is actually
propagated at U2 and U3, but is a computation to determine
that U2 must be stable at the earliest time U3 might change.
This is why an X level should not be latched.
PSpice User's Guide
603
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
In the event that discounting the common ambiguity does not
preclude latching the X (or, in the case of simple gates,
predicting a glitch), the situation is called a reconvergence
hazard. This is the same as a convergence hazard with the
conflicting signal ambiguities having a common origin.
To use digital worst-case simulation effectively, find the areas
of the circuit where signal timing is most critical and use
constraint checkers where appropriate. These devices identify
specific timing violations, taking into account the actual signal
ambiguities (resulting from the elements’ MIN/MAX delay
characteristics). See the online PSpice Reference Guide for
more information about digital primitives.
The most common areas of concern include:
■
data/clock signal relationships
■
clock pulse-widths
■
bus arbitration timing
Signal ambiguities that converge (or reconverge) on wired
nets or buses with multiple drivers may also produce hazards
in a manner similar to the behavior of logic gates. In such
cases, PSpice A/D factors out any common ambiguity before
reporting the existence of a hazard condition.
The use of constraint checkers to validate signal behavior and
interaction in these areas of your design identifies timing
problems early in the design process. Otherwise, a
timing-related failure is only identifiable when the circuit does
not produce the expected simulation results. See
Methodology on page 606 for information on digital
worst-case timing simulation methodology.
604
PSpice User's Guide
Product Version 10.5
Identification of timing hazards
Glitch suppression due to inertial delay
Signal propagation through digital primitives is performed by
the simulator subject to constraints such as the primitive’s
function, delay parameter values, and the frequency of the
applied stimulus. These constraints are applied both in the
context of a normal, well-behaved stimulus, and a stimulus
that represents timing hazards.
Timing hazards may not necessarily result in the prediction of
an X or glitch output from a primitive; these are due to the
delay characteristics of the primitive, which PSpice A/D
models using the concept of inertial delay.
A device presented with a combination of rising and falling
input transitions (assuming no other dominant inputs)
produces a glitch due to the uncertainty of the arrival times of
the transitions (see Figure 16-13).
Figure 16-13 Glitch suppression example one.
However, when the duration of the conflicting input stimulus is
less than the inertial delay of the device, the X result is
automatically suppressed by the simulator because it would
be overly pessimistic (see Figure 16-14).
Figure 16-14 Glitch suppression example two.
In the analysis of reconvergent fanout cases (where common
ambiguity is recognized), it is possible that conflicting signal
ambiguities may still overlap at the inputs to a primitive, even
after factoring out the commonality. In such cases, where the
PSpice User's Guide
605
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
amount of overlap is less than the inertial delay of the device,
the prediction of a glitch is also suppressed by the simulator
(see Figure 16-15).
TPLHMN=40
TPLHMX=60
55
15
90
30
TPLHMN=4
TPLHMX=10
TPLHMN=10
TPLHMX=45
25
75
Figure 16-15 Glitch suppression example three.
In this case, factoring out the 15nsec common ambiguity still
results in a 5nsec overlap of conflicting states. The glitch is
suppressed, however, because 5nsec is less than
TPLHMX-TPLHMN (the computed inertial delay value of the
AND gate, 6nsec).
Note: Glitch suppression can be overridden by setting the
pulse-width rejection threshold parameter (TPWRT) in
the device’s I/O Model.
Methodology
Note: This is not intended to be a comprehensive discussion
of the application of digital worst-case timing simulation
in the design process. Rather, it is a suggested starting
point for understanding the results of your simulation.
Combining component tolerances and the circuit design’s
functional response to a specific stimulus presents a
challenge. You must make sure that all the finished circuits will
operate properly. Well-designed systems have a high degree
of immunity from the effects of varying combinations of
individual component tolerances.
Digital worst-case timing simulation can help identify design
problems, depending upon the nature of the stimulus applied
to the design. You can use the simulation of signal
propagation through the network to observe the timing
606
PSpice User's Guide
Product Version 10.5
Methodology
relationships among various devices and make adjustments
to the design.
Digital worst-case timing simulation does not yield such
results without an applied stimulus; it is not a static timing
analysis tool. The level of confidence that you establish for
your design’s timing-dependent characteristics is directly a
function of the applied stimulus.
Generally, the most productive way to define a stimulus is to
use functional testing: a stimulus designed to operate the
design in a normal manner, exercising all of the important
features in combination with a practical set of data. For
example, if you were designing a digital ADDER circuit, you
would probably want to ensure that no timing race conditions
existed in the carry logic.
Your timing simulation methodology should include these key
steps:
■
Accurate specification of device delay characteristics.
■
Functional specification of circuit behavior, including all
“don’t care” states or conditions.
■
A set of stimuli designed to verify the operation of all
functions of the design.
One common design verification strategy is stepwise
identification of the sections of the design that are to be
exercised by particular subsets of the stimulus, followed by
verification of the response against the functional
specification.
Complete this phase using normal (not digital worst-case)
simulation, with typical delays selected for the elements. The
crucial metric here is the state response of the design. Note
that (with rare exception) this response consists of defined
states and does not include X’s.
The second phase of design verification is to use digital
worst-case simulation, reapplying the functionally correct
stimulus, and comparing the resulting state response to that
obtained during normal simulation. For example, in the case
of a convergence or reconvergence hazard, look for conflicting
PSpice User's Guide
607
Chapter 16
Digital worst-case timing analysis
Product Version 10.5
rise/fall inputs. In the case of cumulative ambiguity, look for
successive ambiguity regions merging within two edges
forming a pulse. Investigate differences at primary
observation points (such as circuit outputs and internal state
variables)—particularly those due to X states (such as critical
hazards)—to determine their cause.
Starting at those points, use the waveform analyzer and the
circuit schematic to trace back through the network. Continue
until you find the reason for the hazard.
After you identify the appropriate paths and know the relative
timing of the paths, you can do either of the following:
■
Modify the stimulus (in the case of a simple convergence
hazard) to rearrange the relative timing of the signals
involved.
Note: Modifying the stimulus is not generally effective for
reconvergent hazards, because the problem is between
the source of the reconvergent fanout and the location of
the hazard. In this case, discounting the common
ambiguity did not preclude the hazard.
■
Change one or both of the path delays to rearrange the
relative timing, by adding or removing logic, or by
substituting component types with components that have
different delay characteristics.
In the case of the cumulative ambiguity hazard, the most likely
solution is to shorten the path involved. You can do this in
either of two ways:
608
■
Add a synchronization point to the logic, such as a
flip-flop—or gating the questionable signal with a clock
(having well-controlled ambiguity)—before its ambiguity
can grow to unmanageable duration.
■
Substitute faster components in the path, so that the
buildup of ambiguity happens more slowly.
PSpice User's Guide
Part four: Viewing results
Part four describes the ways to view simulation results.
PSpice User's Guide
■
Chapter 17, “Analyzing waveforms,” describes how to
perform graphical waveform analysis of simulation
results.
■
Chapter 18, “Measurement expressions,” describes how
to put together measurement expressions using the
measurement definitions included with PSpice. The
Power Users section includes instructions on how to
compose your own measurement definitions.
■
Chapter 19, “Other output options,” describes the special
symbols you can place on your schematic to generate
additional information to the PSpice output file, PSpice
window, and to digital test vector files.
609
Chapter
610
Part four: Viewing results
Product Version 10.5
PSpice User's Guide
Analyzing waveforms
17
Chapter overview
This chapter describes how to perform graphical waveform
analysis of simulation results in PSpice. This chapter includes
the following:
PSpice User's Guide
■
Overview of waveform analysis on page 612
■
Setting up waveform analysis on page 617
■
Viewing waveforms on page 622
■
Viewing large data files on page 650
■
Using simulation data from multiple files on page 658
■
Analog example on page 665
■
Mixed analog/digital tutorial on page 669
■
User interface features for waveform analysis on
page 674
■
Tracking digital simulation messages on page 687
■
Trace expressions on page 689
611
Chapter 17
Analyzing waveforms
Product Version 10.5
Overview of waveform analysis
You can use the waveform analysis features of PSpice to
visually analyze and interactively manipulate the waveforms
generated from the simulation data.
PSpice uses high-resolution graphics so you can view the
results of a simulation both on the screen and in printed form.
On the screen, waveforms appear as plots displayed in Probe
windows within the PSpice workspace.
In effect, waveform analysis is a software oscilloscope.
Performing a PSpice simulation corresponds to building or
changing a breadboard, and performing waveform analysis
corresponds to looking at the breadboard with an
oscilloscope.
With waveform analysis you can:
■
View simulation results in multiple Probe windows
■
Compare simulation results from multiple circuit designs
in a single Probe window
■
Display simple voltages, currents, and noise data
■
Display complex arithmetic expressions that use the
basic measurements
■
Display Fourier transforms of voltages and currents, or of
arithmetic expressions involving voltages and currents
■
For mixed analog/digital simulations, display analog and
digital waveforms simultaneously with a common time
base
■
Add text labels and other annotation symbols for
clarification
PSpice generates two forms of output: the simulation output
file and the waveform data file. The calculations and results
reported in the simulation output file act as an audit trail of the
simulation. However, the graphical analysis of information in
the waveform data file is the most informative and flexible
method for evaluating simulation results.
612
PSpice User's Guide
Product Version 10.5
Chapter overview
Elements of a plot
A single plot consists of the analog (lower) area and the digital
(upper) area.
digital
area
analog
area
Figure 17-1 Analog and digital areas of a plot.
You can display multiple plots simultaneously. If you display
only analog waveforms, the entire plot will be an analog area.
Likewise, if you display only digital waveforms, the entire plot
will be a digital area.
PSpice User's Guide
613
Chapter 17
Analyzing waveforms
Product Version 10.5
Elements of a Probe window
A Probe window is a separately managed waveform display
area. A Probe window can include multiple analog and digital
plots. Figure 17-2 shows two plots displayed together.
Because a Probe window is a window object, you can
minimize and maximize windows, or move and scale the
windows, within the PSpice workspace. The toolbar in the
Probe window applies to the active window.
Tip
From the View menu, choose Toolbar to display or
hide the toolbar.
window A
window B
(active)
Figure 17-2 Two Probe windows.
You can display information from one or more waveform data
files in one Probe window. After the first file is loaded, you can
load other files into the same Probe window by appending
them in PSpice (using the Append Waveform command under
the File menu).
614
PSpice User's Guide
Product Version 10.5
Chapter overview
Managing multiple Probe windows
You can open any number of Probe windows. Each Probe
window is a tab on the worksheet displayed in the middle of
the workspace.
The same waveform data file can be displayed in more than
one Probe window. You can tile the windows to compare data.
Only one Probe window is active at any given time. It is
identified by a highlighted title bar or a topmost tab. Menu,
keyboard, and mouse operations affect only the active Probe
window. You can switch to another Probe window by clicking
another tab or title bar.
Printing multiple windows
You can print all or selected Probe windows, with up to nine
windows on a single page. When you choose Print from the
File menu, a list of all open Probe windows appears. Each
Probe window is identified by the unique identifier in
parentheses in its title bar.
The arrangement of Probe windows on the page can be
customized using the Page Setup dialog box. You can print in
either portrait (vertical) or landscape (horizontal) orientation.
You can also use Print Preview to view all of the Probe
windows as they will appear when printed.
Toggling between display modes
You can choose from two different display modes in PSpice:
default and alternate.
The default display mode in PSpice includes the main Probe
window, plus the output window and the simulation status
window. This provides all possible information about the
simulation run and contains all of the toolbars and settings.
The alternate display mode shows only the Probe window with
any waveforms that have been plotted. This mode gives you
only the plots you are interested in seeing without the
additional simulation data normally provided by PSpice. By
PSpice User's Guide
615
Chapter 17
Analyzing waveforms
Product Version 10.5
default, the alternate display mode is set to be visible at all
times.
The toolbar and window settings are saved for each mode.
Any changes you make in the settings will become the new
default the next time you choose that display mode.
The alternate display mode can be very handy when you want
to see the waveforms superimposed on the schematic
diagram for easy debugging and testing of the circuit. You can
customize the alternate display mode to view various toolbars
or other PSpice windows, according to your own preferences.
To toggle between the standard and the alternate display
modes
1
From the View menu, choose Alternate Display or click
the Alternate Display toolbar button.
Keeping the Probe window visible at all times
Like any other application running under Windows, the PSpice
window will remain in the forefront of the desktop only as long
as it is the active window. In order to keep the PSpice window
visible at all times, you can use the push pin feature.
By keeping the Probe window on top of other active windows,
you can easily view the schematic page at the same time you
see the corresponding waveform for that circuit. This allows
you to cross-probe quickly and easily without having to
activate the Probe window each time.
Note: The push pin button is a toggle: clicking on it when it is
enabled will disable the “on top” function.
To make the Probe window visible at all times
1
616
Click the push pin button in the toolbar.
PSpice User's Guide
Product Version 10.5
Chapter overview
Setting up waveform analysis
Setting up colors
You can configure Probe display and print colors in:
■
The configuration file, PSPICE.INI
■
The Probe Options dialog box
For information on how to use the available colors and color
order in a Probe window, see Configuring trace color schemes
on page 620.
Editing display and print colors in the PSPICE.INI file
In the file, you can control the following print and display color
settings for Probe windows:
■
The colors used to display traces
■
The colors used for the Probe window foreground and
background
■
The order colors are used to display traces
■
The number of colors used to display traces
To edit display and print colors in the PSPICE.INI file
Note: After editing PSPICE.INI, you must restart PSpice
before your changes will take effect.
PSpice User's Guide
1
In a standard text editor (such as Notepad), open
PSPICE.INI. (This file should be located in the
\tools\PSpice directory under the main OrCAD program
installation.)
2
Scroll to the [PROBE DISPLAY COLORS] or
[PROBE PRINTER COLORS] section of the file.
3
Add or modify a color entry. See Table 17-1 on page 619
for a description of color entries and their default values.
617
Chapter 17
Analyzing waveforms
Product Version 10.5
Colors for all items are specified as
<item name>=<color>.
The item names and what they represent are listed in
Table 17-1 on page 619. Valid item names include:
❑
BACKGROUND
❑
FOREGROUND
❑
TRACE_1 through TRACE_12
Here are the color names you can specify:
4
618
black
blue
brightblue
brightcyan
brightgreen
brightmagenta
brightred
brightwhite
brightyellow
brown
cyan
darkblue
darkcyan
darkgray
darkgreen
darkmagenta
darkpink
darkred
green
lightblue
lightgray
lightgreen
magenta
mustard
orange
pink
purple
red
white
yellow
If you added or deleted trace number entries, set
NUMTRACECOLORS=n to the new number of traces,
where n is between 1 and 12. This item represents the
number of trace colors displayed on the screen or printed
before the color order repeats.
PSpice User's Guide
Product Version 10.5
Chapter overview
5
Save the file.
Table 17-1 Default waveform viewing colors.
Item Name
Description
Default
BACKGROUND
specifies the color of BLACK
window background
FOREGROUND specifies the default WHITE
color for items not
explicitly specified
TRACE_1
specifies the first
color used for trace
display
TRACE_2
specifies the second BRIGHTRED
color used for trace
display
TRACE_3
specifies the third
color used for trace
display
BRIGHTBLUE
TRACE_4
specifies the fourth
color used for trace
display
BRIGHTYELLOW
TRACE_5
specifies the fifth
color used for trace
display
BRIGHTMAGENT
A
TRACE_6
specifies the sixth
color used for trace
display
BRIGHTCYAN
BRIGHTGREEN
Note: When you want to copy Probe plots to the clipboard
and then paste them into a black and white document,
choose the Change All Colors to Black option under
Foreground in the Copy to Clipboard–Color Filter
dialog box (from the Window menu, choose Copy to
Clipboard).
PSpice User's Guide
619
Chapter 17
Analyzing waveforms
Product Version 10.5
Configuring trace color schemes
In the Probe Options dialog box, you can set options for how
the available colors and the color order specified in the
PSPICE.INI file are used to display the traces in a Probe
window. You can use:
■
a different color for each trace
■
the same color for all the traces that belong to the same
y-axis
■
the available colors in sequence for each y-axis
■
the same color for all the traces that belong to the same
waveform data file
For information on what the default available colors and color
order are and how to change them, see Editing display and
print colors in the PSPICE.INI file on page 617.
To configure trace color schemes in the Probe Options
dialog box
1
620
From the Tools menu, choose Options to display the
Probe Options dialog box.
PSpice User's Guide
Product Version 10.5
Chapter overview
2
Under Trace Color Scheme, choose one of the following
options:
Table 17-2
Choose this option... To do this...
Normal
Use a different color for each trace
(for up to 12 traces, depending on
the number of colors set in the
PSPICE.INI file).
Match Axis
Use the same color for all the traces
that belong to the same y-axis. The
title of the axis (by default, 1, 2, etc.)
is the same color as its traces.
Sequential Per Axis
Use the available colors in
sequence for each y-axis.
Unique by File
Use the same color for all the traces
in one Probe window that belong to
the same waveform data file.
3
Click OK.
PSpice saves the selected color scheme for future
waveform analyses.
PSpice User's Guide
621
Chapter 17
Analyzing waveforms
Product Version 10.5
Viewing waveforms
If you are using Capture, you can either view waveforms
automatically after you run a simulation, or you can monitor
the progress of the simulation as it is running.
You do not need to exit PSpice if you are finished examining
the simulation results for one circuit and want to begin a new
simulation from within Capture. However, PSpice unloads the
old waveform data file for a circuit each time that you run a new
simulation of the circuit. After the simulation is complete, the
new or updated waveform data file is loaded for viewing.
Setting up waveform display from Capture
You can configure the way you want to view the waveforms in
PSpice by defining display settings in the Probe Window tab
in the Simulation Settings dialog box.
The display settings in the Probe Window tab are explained in
the following table.
622
PSpice User's Guide
Product Version 10.5
Chapter overview
Table 17-3
This setting...
Enables this type of waveform display...
Display Probe
window when
profile is
opened.
Waveforms are displayed only when a
.DAT file is opened from within PSpice.
Display Probe
Waveforms are displayed as the
window... during simulation progresses (“marching
simulation.
waveforms”).
Display Probe
window... after
simulation has
completed.
Waveforms are displayed only after the full
simulation has completed and all data has
been calculated.
Show... All
markers on
open
schematics.
Waveforms are displayed for those nets
that have markers attached in the
schematic.
Show... Last
plot.
Waveforms are displayed according to the
last display configuration that was used in
the Probe window.
Show...
Nothing.
No waveforms are displayed.
Viewing waveforms while simulating
While a simulation is in progress, you can monitor the results
for the data section being written by PSpice. This function is
only available when the Display Probe window during
simulation option is enabled in the Probe Window tab of the
Simulation Settings dialog box.
To monitor results during a simulation
PSpice User's Guide
1
From Capture’s PSpice menu, choose Edit Simulation
Profile to display the Simulation Settings dialog box.
2
Click the Probe Window tab.
623
Chapter 17
Analyzing waveforms
Product Version 10.5
3
Select Display Probe window and then click during
simulation.
4
Click OK to close the Simulation Settings dialog box.
5
From the PSpice menu, choose Run to start the
simulation.
One Probe window is displayed in monitor mode.
Note: If you open a new Probe window (from the Window
menu, choose New Window) while monitoring the data,
the new window also starts in monitor mode because it is
associated with the same waveform data file.
Note: During a multi-run simulation (such as Monte
Carlo, parametric, or temperature), PSpice displays only
the data for the most recent run in the Probe window.
6
Do one of the following to select the waveforms to be
monitored:
❑
From PSpice’s Trace menu, choose Add, and enter
one or more trace expressions.
❑
From Capture’s PSpice menu, point to Markers, then
choose and place one or more markers.
For more information, see Using schematic page
markers to add traces on page 626.
The Probe window monitors the waveforms for as long as
the most recent data section is being written. After that
data section is finished, the window changes to manual
mode. To see the full set of runs, you must update the
display by using the Add Trace command under the Trace
menu.
Configuring update intervals
You can define the frequency at which PSpice updates the
waveform display as follows:
624
■
At fixed time intervals (every n sec)
■
According to the percentage of simulation completed
(every n %), where n is user-defined
PSpice User's Guide
Product Version 10.5
Chapter overview
The default setting (Auto) updates traces each time PSpice
gets new data from a simulation.
To change the update interval
1
From the Tools menu, choose Options.
2
In the Auto-Update Interval frame, choose the interval
type (sec or %), then type the interval in the text box.
Interacting with waveform analysis during simulation
The functions that change the x-axis domain (that set a new
x-axis variable) can not be accessed while the simulation is
running. If you have enabled the display of waveforms during
simulation and wish to reconfigure the x-axis settings (as
explained below), you must wait until the simulation run has
finished.
The following table shows how to enable the functions that
change the x-axis domain.
Table 17-4
Enable this function... By doing this...
Fast Fourier transforms
Performance analysis
New x-axis variable
1. From the Plot menu, choose Axis
Settings.
2. In the Processing Options frame,
select Fourier.
1. From the Plot menu, choose Axis
Settings.
2. In the Processing Options frame,
select Performance Analysis.
1. From the Plot menu, choose Axis
Settings, then click the X Axis
tab.
2. Click the Axis Variable button.
3. In the X Axis Variable dialog box,
specify a new x-axis variable.
PSpice User's Guide
625
Chapter 17
Analyzing waveforms
Product Version 10.5
Table 17-4
Enable this function... By doing this...
Goal function evaluation
Load a completed data
section
1. From the Trace menu, select Eval
Goal Function.
2. In the Evaluate Goal Function(s)
dialog box, specify a goal
function.
1. From the File menu, choose
Append Waveform (.DAT).
2. Select a .DAT file to append.
Pausing a simulation and viewing waveforms
You can pause a simulation to analyze waveforms before the
simulation is finished. After you pause the simulation, you can
either resume the simulation or end it.
To pause a simulation
1
From PSpice’s Simulation menu, choose Pause.
2
In the Probe window, view the waveforms generated
before you paused the simulation.
3
Do one of the following:
❑
From the Simulation menu, choose Run to resume
the simulation.
❑
From the Simulation menu, choose Stop to stop the
simulation.
Using schematic page markers to add traces
You can place markers on a schematic page to identify the
nodes for which you want waveforms displayed in Probe. See
Trace expressions on page 689 for ways to add traces within
PSpice.
You can place markers:
626
PSpice User's Guide
Product Version 10.5
Chapter overview
■
Before simulation, to limit results written to the waveform
data file and automatically display those traces in PSpice.
■
During or after simulation, with PSpice A/D running, to
automatically display traces in the active Probe window.
After simulation, the color of the marker you place is the same
as its corresponding waveform analysis trace. If you change
the color of the trace, the color of the marker on the schematic
page changes accordingly.
The Markers submenu also provides options for controlling
the display of marked results in PSpice, after initial marker
placement, and during or after simulation.
Power markers allow you to measure the power dissipation of
a particular device. You can use these markers in the same
way you use current and voltage markers. Power markers are
annotated with “W” and are placed on devices that have
PSpice models. The corresponding power dissipation
waveforms for the devices will be calculated and displayed in
Probe.
Place markers on subcircuit nodes. This allows you to perform
cross-probing between the front-end design entry tool and
PSpice at the lower level circuits of a hierarchical design.
PSpice User's Guide
627
Chapter 17
Analyzing waveforms
Product Version 10.5
To place markers on a schematic page
1
From Capture’s PSpice menu, point to Markers, then
choose the marker type you want to place. (Some of the
markers are from the Advanced submenu.)
Table 17-5
628
Waveform
Markers menu
command
Advanced submenu
command
voltage
Voltage Level
not required
voltage
differential
Voltage Differential not required
current
Current Into Pin
not required
digital signal
Voltage Level
not required
dB1
Advanced
db Magnitude of
Voltage
db Magnitude of
Current
phase1
Advanced
Phase of Voltage
Phase of Current
group delay1
Advanced
Group Delay of Voltage
Group Delay of Current
real1
Advanced
Real Part of Voltage
Real Part of Current
imaginary1
Advanced
Imaginary Part of
Voltage
Imaginary Part of
Current
power
Power Dissipation
not required
PSpice User's Guide
Product Version 10.5
Chapter overview
1. You can use these markers instead of the built-in functions
provided in output variable expressions (see Table 17-18 on
page 700). However, these markers are only available after
defining a simulation profile for an AC Sweep/Noise analysis.
2
Point to the wires or pins you wish to mark and click to
place the chosen markers.
3
Right-click and select End Mode to stop placing markers.
4
If you have not simulated the circuit yet, from the PSpice
menu, choose Run.
After simulation, the color of the marker is the same as its
corresponding waveform analysis trace. If you change the
color of the trace, the color of the marker changes
accordingly.
To hide or delete marked results
1
From Capture’s PSpice menu, point to Markers, then
choose one of the following:
Table 17-6
PSpice User's Guide
Choose this
option...
To do this...
Hide All
Hide traces in the waveform analysis
display for all markers placed on any
page or level of the schematic.
Delete All
Remove all markers from the schematic
and all corresponding traces from the
waveform analysis display.
629
Chapter 17
Analyzing waveforms
Product Version 10.5
Using display control
You can create displays to save the contents of a Probe
window. You can view a display again at a later time with a
different simulation so long as the new simulation has
identically named variables.
Once the display is saved, you can copy it, edit it, and delete it.
To save a display
1
Set up the plots, traces, labels, and axes in the Probe
window you want to save.
2
From the Window menu, choose Display Control.
The Display Control dialog box appears.
630
3
Click on the Displays tab.
4
In the New Name text box, type a name for the display.
5
Do one of the following:
❑
To save the display in the current .PRB file, click
Save.
❑
To save the display in another .PRB file, click Save
To. Specify the name and location of the file. Click
OK.
PSpice User's Guide
Product Version 10.5
Chapter overview
6
Click Close.
To copy a display
1
From the Window menu, choose Display Control.
The Display Control dialog box appears.
2
Click on the Displays tab.
3
Click the name of the display to copy.
4
Click Copy To.
5
Specify the name and location of the copied display.
6
Click OK.
7
Click Close.
To delete a display
1
From the Window menu, choose Display Control.
The Display Control dialog box appears.
2
Click on the Displays tab.
3
Do one of the following:
4
❑
To delete a display from the current .PRB file, click
the name, then click Delete.
❑
To delete a display from a global or remote .PRB file,
click Delete From, then select the .PRB file.
Click Close.
To use a saved display
1
From the Window menu, choose Display Control.
The Display Control dialog box appears.
2
Click on the Displays tab.
3
Do one of the following:
❑
PSpice User's Guide
To use a display listed here, click the name.
631
Chapter 17
Analyzing waveforms
Product Version 10.5
❑
4
To use a display from another .PRB, click Load.
Select the file. Click OK. Click the name of the
display.
Click Restore.
Note: You can use a saved display to display traces as long
as the current data file has variables with the same
names as the variables in the display file.
To load displays from another .PRB file
1
From the Window menu, choose Display Control.
The Display Control dialog box appears.
632
2
Click on the Displays tab.
3
Click Load.
4
Select the file.
5
Click OK.
PSpice User's Guide
Product Version 10.5
Chapter overview
Using plot window templates
PSpice provides plot window templates that allow you to
create and reuse custom displays in Probe using defined
arguments. A plot window template is a plot window consisting
of one or more arguments used to represent node voltage, pin
current, power or digital names within a display. An argument
provides the means to replace a fixed node voltage or pin
current name with a node voltage or pin current name you
choose.
You can create unique plot window templates for a particular
design or general templates that can be applied to various
designs. A set of some of the more commonly used templates
are predefined and included with PSpice.
To work with plot window templates, from the Window menu,
choose Display Control, and click the Templates tab. Here you
can customize plot window templates in various ways.
Creating a plot window template
In order to create and save a new plot window template, you
must first set up the active plot window in Probe with the
configuration you want. The active plot window will be the
basis for the template properties you save.
PSpice User's Guide
633
Chapter 17
Analyzing waveforms
Product Version 10.5
Note: A plot window template that is saved to a simulation
profile that you define cannot be used with markers in
OrCAD Capture. The list of plot window templates
displayed in PSpice includes user-defined templates,
but the list in OrCAD Capture does not show these. To
view user-defined templates in OrCAD Capture, you
must copy the templates to either the local or global
.PRB file.
To create a new plot window template
634
1
In PSpice, from the Window menu, choose Display
Control.
2
Click the Templates tab.
3
In the New Name text box, enter the name for the new
template you want to create.
4
Click Save or Save To.
PSpice User's Guide
Product Version 10.5
Chapter overview
The Save Plot Window Template – Step 1 of 2 dialog box
appears.
5
In the Description text box, type in a description for the
template, if you would like one. (This is optional.)
6
If you clicked Save To, choose the .PRB file you wish to
save the template to by selecting the appropriate radio
button under the Save Template In frame. (The default is
the local .PRB file. For the Save function, the Local File is
the only option.)
7
PSpice User's Guide
❑
Local File – the .PRB file for the current simulation in
PSpice.
❑
Global File – the .PRB file to be used globally for all
Probe displays.
❑
Other File – another .PRB file stored elsewhere on
your hard disk or network drive. Use the Browse
button to locate the file on a particular drive.
Click the Next> button.
635
Chapter 17
Analyzing waveforms
Product Version 10.5
The Save Plot Window Template – Step 2 of 2 dialog box
appears. The number of Node/Pin Name arguments that
are listed here is determined by the current display.
8
Define the association of each argument by selecting the
node or pin name from the drop-down list under the
column Node/Pin Name.
This drop-down list shows all of the available node
voltage, pin current, power or digital names. If the
drop-down list does not appear, click in the text box to
activate the drop-down button.
9
For each argument, set the Type of argument to be used
by selecting the argument name from the drop-down list
under the column Type.
This drop-down list shows all of the available argument
types (any, current, power, voltage). If the drop-down list
does not appear, click in the text box to activate the
drop-down button.
10 For each argument, under the Description column, type in
a description for the argument, if you would like one. (This
is optional.)
The description you enter here will be displayed in the
status line of Capture when placing a marker associated
with the argument.
11 If desired, change the order of the arguments by using the
Arrow buttons to move an argument up or down in the
listing. Or, you can delete an argument by selecting it and
clicking the Delete button.
636
PSpice User's Guide
Product Version 10.5
Chapter overview
12 Click Finish.
Note: At least one argument is required to create a plot
window template. The maximum number of arguments
allowed is the number of unique node voltage, pin
current, power or digital names in the active display.
Modifying a plot window template
Modifying a plot window template is essentially the same as
creating a new template. In order to modify a plot window
template, that particular template must be the active plot
window in Probe. If the active display is not the template you
want to modify, use the Restore button to make a different
template the active display in Probe
To modify a plot window template
PSpice User's Guide
1
From the Window menu, choose Display Control.
2
Click the Templates tab.
3
Select the template you want to modify by clicking on its
name in the list of loaded templates. If the template you
are looking for is not in the list, use the Restore button to
make it the active display.
637
Chapter 17
Analyzing waveforms
Product Version 10.5
4
Click the Save button to display the Save Plot Window
Template – Step 1 of 2 dialog box.
5
Make the desired changes, then click Next to display the
Save Plot Window Template – Step 2 of 2 dialog box.
6
Make the desired changes, then click Finish.
The modifications will be saved and the display will be
updated automatically.
Note: If an argument assignment no longer applies because
the node voltage, pin current, power or digital names
are mapped to an argument that has changed, then
information regarding that argument will not be
available in the Step 2 of 2 dialog box.
638
PSpice User's Guide
Product Version 10.5
Chapter overview
Deleting a plot window template
You can easily delete a plot window template from the list of
loaded templates. This does not erase the template from your
system. It only removes it from the list of templates you can
access and erases it from the .PRB file.
To delete a plot window template
1
From the Window menu, choose Display Control.
2
Click the Templates tab.
3
Click on the name of the plot window template you want
to delete.
4
Click Delete.
Copying a plot window template
You can copy a plot window template into another .PRB file to
make it available for use later with that file.
To copy a plot window template
1
From the Window menu, choose Display Control.
2
Click the Templates tab.
3
Click on the name of the plot window template you want
to copy.
4
Click Copy To.
The Probe File for Save Template dialog box appears.
5
PSpice User's Guide
Choose the .PRB file you wish to save the template to by
selecting the appropriate radio button under the Save
Template In frame. (The default is the local .PRB file.)
❑
Local File – the .PRB file for the current simulation in
PSpice.
❑
Global File – the .PRB file to be used globally for all
Probe displays.
639
Chapter 17
Analyzing waveforms
Product Version 10.5
❑
6
Other File – another .PRB file stored elsewhere on
your hard disk or network drive. Use the Browse
button to locate the file on a particular drive.
Click OK.
Restoring a plot window template
In order to make a plot window template the active display in
Probe, you must restore it. This process recalls a previously
defined plot window template and sets up a new plot window
in Probe using the arguments associated with that template.
In order for the arguments in the template to apply, you must
replace the node voltage names or pin current names for each
argument contained in the restored template.
Note: You can only restore plot window templates that are
already loaded. If you want to restore a plot window
template that does not appear in the list, you must first
load it.
To restore a plot window template
640
1
From the Window menu, choose Display Control.
2
Click the Templates tab.
3
Click Restore.
PSpice User's Guide
Product Version 10.5
Chapter overview
The Restore Plot Window Template dialog box appears.
4
Reassign the node voltage names or pin current names
for each argument in the list.
5
Click OK.
A new Probe window will be created and the restored plot
window template will be displayed.
Note: You may also restore a plot window template by
choosing the Add Trace command from the Trace
menu, and then selecting Plot Window Templates from
the drop-down list in the Functions or Macros frame.
Viewing the properties of a plot window template
You can view the properties of a plot window template and
change the description fields for the template or arguments it
contains.
Note: A plot window template that is saved to a simulation
profile that you define cannot be used with markers in
OrCAD Capture. The list of plot window templates
displayed in PSpice includes user-defined templates,
but the list in OrCAD Capture does not show these. To
view user-defined templates in OrCAD Capture, you
PSpice User's Guide
641
Chapter 17
Analyzing waveforms
Product Version 10.5
must copy the templates to either the local or global
.PRB file.
To view the properties of a plot window template
1
From the Window menu, choose Display Control.
2
Click the Templates tab.
3
Click on the name of the plot window template you want
to view.
4
Click Properties.
The Plot Window Template Properties dialog box
appears.
5
Change the Description field for the template, or change
the description for any of the Arguments, as desired.
6
Click Finish to exit and save any changes.
Note: When viewing the properties of a template, you can
only edit the description fields. No other changes are
allowed. If you want to modify the arguments or
assignments, you need to modify the template.
642
PSpice User's Guide
Product Version 10.5
Chapter overview
Loading a plot window template
You can load a plot window template from another .PRB file,
and add it to the list of available templates. When you load a
template, you do not make it the active display in Probe. You
are only adding it to the list of available templates. (To view the
newly loaded template, you need to restore it.)
If a duplicate template is loaded, then the one you are loading
will replace the current one in the list. If you close the data file
and reopen it, any plot window templates that you loaded
earlier will have to be loaded again to make them available.
(Loaded templates are not saved with the data file.)
To load a plot window template
1
From the Window menu, choose Display Control.
2
Click the Templates tab.
3
Clck Load.
The Load Displays dialog box appears.
4
Locate the .PRB file that contains the plot window
template you want to load.
5
Select the file and then choose Open.
The loaded templates will be listed in the Display Control
dialog box.
Placing plot window template markers in Capture
Place a marker in Capture that represents a plot window
template. The marker will restore the associated template
when you run the simulation in PSpice. Markers for plot
window templates are distinguished from other markers (for
PSpice User's Guide
643
Chapter 17
Analyzing waveforms
Product Version 10.5
voltage, current, or power) by being square rather than round
in shape.
A simulation profile must be active in order to place a marker
for a plot window template. The analysis type defined in the
profile will determine what type of template will be loaded
(either for AC, DC or transient analysis).
When placing a plot window template marker, the argument
description for the template being placed will appear in the
status bar of Capture. Markers will continue to be placed until
all arguments for the template have been satisfied. If an active
simulation exists, then the template markers will turn black;
otherwise, they will remain gray.
If an argument type is set to "Any" rather than a specific type,
the marker type will depend on the marker placement location.
If a marker is placed on a pin, then it will be assumed to be a
current marker. If a marker is placed on a node, it will be
assumed to be a voltage marker. If a marker is placed on a
device, it will be assumed to be a power marker.
To place a plot window template marker
1
644
In Capture, from the PSpice menu, choose Markers, then
select Plot Window Templates.
PSpice User's Guide
Product Version 10.5
Chapter overview
The Plot Window Templates dialog box appears.
2
Click on the template you want to associate with the
marker you will place.
3
Click the Place button.
A plot window template marker will appear and be
attached to the cursor.
4
Place the marker at a particular location on the schematic
page.
5
Continue to place markers at the appropriate locations
until all the arguments for the template have been
satisfied.
Note: PSpice does not have to be running in order for you to
place a marker for a plot window template. The list of
loaded templates comes from either the default
PSPICE.PRB file or from the .PRB file for the active
profile, if that exists.
Caution
Plot Window Templates are displayed properly
only if one template is added at a time. Therefore,
in a situation where multiple Plot Window
Templates are added before simulation, all the
PSpice User's Guide
645
Chapter 17
Analyzing waveforms
Product Version 10.5
templates will be ignored. In cases where
simulation is done first and markers are added
later on, every thing works fine, since only one
Plot Window Template gets added at a time.
Limiting waveform data file size
When PSpice performs a simulation, it creates a waveform
data file. The size of this file for a transient analysis is roughly
equal to:
(# transistors)·(# simulation time points)·24 bytes
The size for other analysis types is about 2.5 times smaller.
For long runs, especially transient runs, this can generate
waveform data files that are several megabytes in size. Even
if this does not cause a problem with disk space, large
waveform data files take longer to read in and take longer to
display traces on the screen.
You can limit waveform data file size by:
■
placing markers on your schematic before simulation and
having PSpice restrict the saved data to these markers
only
■
excluding data for internal subcircuits
■
suppressing simulation output
Limiting file size using markers
One reason that waveform data files are large is that, by
default, PSpice stores all net voltages and device currents
for each step (for example, time or frequency points).
However, if you have placed markers on your schematic prior
to simulation, PSpice can save only the results for the marked
wires and pins.
646
PSpice User's Guide
Product Version 10.5
Chapter overview
To limit file size using markers
1
From Capture’s PSpice menu, choose Edit Simulation
Profile to display the Simulation Settings dialog box.
2
Click the Data Collection tab.
3
In the Data Collection Options frame, choose the desired
option for each type of marker (Voltages, Currents,
Power, Digital, Noise).
Table 17-7
PSpice User's Guide
Option
Description
All
All data will be collected and stored.
(This is the default setting.)
All but Internal
Subcircuits
All data will be collected and stored
except for internal subcircuits of
hierarchical designs (top level data only).
At Markers only
Data will only be collected and stored
where markers are placed.
None
No data will be collected.
4
Check the Save data in the CSDF format (.CSD) if you
want the data to be stored in this format.
5
Click OK to close the Simulation Settings dialog box.
647
Chapter 17
Analyzing waveforms
Product Version 10.5
6
From the PSpice menu, point to Markers, then choose the
marker type you want to place.
The color of the marker on the schematic page is the
same as its corresponding waveform analysis trace. If
you change the color of the trace, the color of the marker
changes accordingly.
7
Point to the wires or pins you wish to mark and click to
place the chosen markers.
8
Right-click and select End Mode to stop placing markers.
9
From the PSpice menu, choose Run to start the
simulation.
When the simulation is complete, the corresponding
waveforms for the marked nodes or devices will be
displayed in Probe.
Limiting file size by excluding internal subcircuit data
By default, PSpice saves data for all internal nodes and
devices in subcircuit models in a design. You can exclude data
for internal subcircuit nodes and devices.
648
PSpice User's Guide
Product Version 10.5
Chapter overview
To limit file size by excluding data for internal subcircuits
1
From the Capture PSpice menu, choose Edit Simulation
Profile to display the Simulation Settings dialog box.
2
Click the Data Collection tab.
3
In the Data Collection Options frame, choose All but
Internal Subcircuits for each marker type.
4
Click OK to close the Simulation Settings dialog box.
5
From the PSpice menu, choose Run to start the
simulation.
Limiting file size by suppressing the first part
of simulation output
Long transient simulations create large waveform data files
because PSpice stores many data points. You can suppress a
part of the data from a transient run by setting the simulation
analysis to start the output at a time later than 0. This does not
affect the transient calculations themselves—these always
start at time 0. This delay only suppresses the output for the
first part of the simulation.
Note: Suppressing part of the data from a run also limits the
size of the PSpice output file.
PSpice User's Guide
649
Chapter 17
Analyzing waveforms
Product Version 10.5
To limit file size by suppressing the first part of transient
simulation output
1
From Capture’s PSpice menu, choose Edit Simulation
Profile to display the Simulation Settings dialog box.
2
Click the Analysis tab.
3
From the Analysis type list, select the
Time Domain (Transient) option.
4
In the Start saving data after text box, type a delay time.
5
Click OK to close the Simulation Settings dialog box.
6
From the PSpice menu, choose Run to start the
simulation.
The simulation begins, but no data is stored until after the
delay has elapsed.
Viewing large data files
At times there are situations where you cannot reduce the size
of the data file being generated, but would like to load large
data files on to the Probe for viewing the trace.
As PSpice depends on system memory for loading and
displaying any trace, if the data file is so large that cannot be
loaded, the trace does not get displayed at all. Usually data
files with size greater than 2 GB are considered to be large
data files. Whether a data file can be categorized as large
depends on the size of the data file and the number of traces
within the data file. For example, a data file that has 10 traces
and is of 2 GB may not be a large data file. But if a data file
has single trace and is of 2 GB or more, it can be termed as a
large data file.
Important
By default, any data file with more than 1 million data
points per trace is considered as large data file by
PSpice.
To load and view data files with more than 1 million data
points, PSpice provides you with the following options.
650
PSpice User's Guide
Product Version 10.5
Chapter overview
■
Displaying fewer data points
■
Displaying partial trace
Displaying fewer data points
If a data file is too large to be loaded on to PSpice, you can
choose to display the complete trace that has been created
using a fewer data points.
For example, if the complete trace uses 3 million data points,
the trace displayed on the probe window will be created using
only 1 million data points.
In this option though the complete trace is displayed, it is not
very accurate. The number of data points used to construct
the complete trace depends on the system memory available
for loading data points. By default, the limit is set to 1 million
data points per part of the trace. If required you can increase
this limit. For more information see, Changing threshold for
large data file.
Displaying partial trace
Another method of loading and displaying a large data file on
to PSpice, is to break the complete trace into multiple smaller
PSpice User's Guide
651
Chapter 17
Analyzing waveforms
Product Version 10.5
parts. You can then view each part separately in the PSpice
probe window. See the figure below.
Complete Trace
Complete trace broken in 5 parts
Part 1 of
the trace
Part 5 of
the trace
Part 2 of
the trace
Part 3 of
the trace
Part 4 of
the trace
Figure 17-3 Displaying partial traces
Number of parts into which the complete trace can be divided
is governed by the number of data points in the trace.
For example, if a complete trace has 4.5 million data points,
and at any given point of time PSpice is configured to load only
1 million data points, the complete trace will be divided into 5
parts. First four part traces will be of 1 million data points each
and the last part trace will be of 500000 data points.
The size of the partial trace is also influenced by the number
of data points per part. By default, the limit is set to 1 million
data points per part of the trace. If required you can increase
652
PSpice User's Guide
Product Version 10.5
Chapter overview
this limit. For more information see, Changing threshold for
large data file.
When you display partial traces, marching waveforms are not
supported.
Select this to
load the next
part of the trace
You can also use the Load Next Part button in the Probe
toolbar for loading and viewing the next part of the trace. The
PSpice User's Guide
653
Chapter 17
Analyzing waveforms
Product Version 10.5
down-arrow button is used to display the next 5 or the previous
5 parts of the trace or both as the case may be.
Load Next Part
Down-arrow
button
Tool button for loading and
viewing any part of the
Loading a large data file
If you are trying to open a large data file in PSpice, the Large
Data File dialog box appears.
To load and display the data file, you can either select the Use
fewer data points to display complete trace option or the
Use all data points to display trace in parts option.
654
PSpice User's Guide
Product Version 10.5
Chapter overview
To load the complete data file, select the Ignore this warning
option. When you select this option, the data file may or may
not get loaded depending on your system memory.
For example, on some machines a data file with 5 million data
points may open without any problems while on some other
machine the same data file might be too large to be loaded in
one go.
To make your selection the default setting, select the Always
use this option check box. Once this check box is selected,
next time when you try to open a large data file, the Large Data
File dialog box does not appear. Instead, the option selected
by you previously is used to open the large data file.
Switching Modes
While viewing the trace from a large data file, you can switch
from one mode to another using one of the following methods.
■
Using the View drop-down menu
a. From the View menu in PSpice select Large Data
File Mode.
b. In the Large Data File Mode submenu, select the
mode in which you want to view the trace. The mode
currently selected, has a check mark against it.
■
PSpice User's Guide
❍
Select Display Fewer Data Points when you
want to view the complete trace that may not be
very accurate.
❍
Select Display in parts when you want to view
the partial but an accurate representation of the
trace.
Using the toolbar
655
Chapter 17
Analyzing waveforms
Product Version 10.5
a. To switch modes, select the Toggle Large Data
File Mode button in the Probe toolbar.
Toggle Large Data
File Mode
Changing threshold for large data file
By default, in PSpice any data file with more than 1 million
data points is categorized as a large data (.dat) file. As a
user you can modify this threshold by specifying a higher the
number of data points in the Probe Settings dialog box.
Important
You cannot reduce the limit to lower than 1 million
data points.
To increase the number of data points complete the following
steps:
1
From the Tools menu is PSpice choose Options.
Note: This option is enabled only if a .dat or .sim file
is open in PSpice.
656
PSpice User's Guide
Product Version 10.5
Chapter overview
2
Select the Large Data File tab.
3
In the Data points in one part text box specify the
desired number of data points and click OK.
The changes you have made in the Probe Setting dialog
box, will be effective from the next session.
Caution
Any changes to the threshold for defining large
data file should be made keeping in account your
system memory so as to avoid failure in opening
data files. For example, on a machine low on
system memory, a data file or a part of data file
with 2 million data points might fail to open. On
the other hand, for a high-end machine a limit of
3 million data points might work fine.
PSpice User's Guide
657
Chapter 17
Analyzing waveforms
Product Version 10.5
Using simulation data from multiple files
You can load simulation data from multiple files into the same
Probe window by appending waveform data files.
When more than one waveform data file is loaded, you can
add traces using all loaded data, data from only one file, or
individual data sections from one or more files.
Appending waveform data files
To append a waveform data file
1
In PSpice, from the File menu, choose
Append Waveform (.DAT).
2
Select a *.DAT file to append, and click OK.
3
If the file has multiple sections of data for the selected
analysis type, the Available Sections dialog box appears.
Do one of the following:
4
658
❑
Click the sections you want to use.
❑
Click the All button to use all sections.
Click OK.
PSpice User's Guide
Product Version 10.5
Chapter overview
Importing traces
Besides using the simulation data from .DAT files, you can
also import trace information stored in other file formats. Using
PSpice you can import the traces stored in a tabular format in
a .txt file or a .csv file.
Traces in tabular format
To import a trace
1
From the File drop-down menu choose Import.
2
In the Import File dialog box, select the text file to be
imported in PSpice.
The Import Traces dialog box appears. All the nodes
listed in the source file are listed in the X-axis drop-down
list and the Available Nodes list.
3
In the Import Traces dialog box, specify the name and the
location of the .DAT file in which the imported trace is to
be stored.
4
From the X-Axis drop-down list box, select the node name
to be plotted on the X-Axis.
5
Specify a name for the X-axis. Select one of the following
options for naming the X-axis.
a. Time
PSpice User's Guide
659
Chapter 17
Analyzing waveforms
Product Version 10.5
b. Frequency
c. Sweep Variable: When you select Sweep Variable,
you need to specify the variable name in the enabled
text box.
660
6
From the Available Traces list box, select the traces that
are to be imported in PSpice.
7
Click Add.
8
The selected traces appear in the Import Trace list box. To
import all the traces available in the source file, click the
Add All.
9
Select OK to import the selected trace(s) into the
specified data file.
PSpice User's Guide
Product Version 10.5
Chapter overview
Important
Renaming of X-axis is useful when you want to
import a trace and append it to an existing data file
for comparing traces. To be able to append two
traces successfully, you need to ensure that for both
the traces the range and the name of the variable
plotted on the X-axis should be same.
Adding traces from specific loaded waveform data files
If two or more waveform data files have identical simulation
output variables, trace expressions that include those
variables generate traces for each file. However, you can
specify which waveform data file to use in the trace
expression. You can also determine which waveform data file
was used to generate a specific trace.
To add a trace from a specific loaded waveform data file
1
In PSpice, from the Trace menu, choose Add Trace to
display the Add Traces dialog box.
The Simulation Output Variables list in the Add Traces
dialog box contains the output variables for all loaded
waveform data files.
2
In the Trace Expression text box, type an expression
using the following syntax:
trace_expression@fn
where n is the numerical order (from left to right) of the
waveform data file as it appears in the PSpice title bar, or
trace_expression@s@fn
where s is a specific data section of a specific waveform
data file.
Example: To plot the V(1) output for data section 1 from
the second data file loaded, type the following trace
expression:
V(1)@1@f2
PSpice User's Guide
661
Chapter 17
Analyzing waveforms
Product Version 10.5
You can also use the name of the loaded data file to
specify it. For example, to plot the V(1) output for all data
sections of a loaded data file, MYFILE.DAT, type the
following trace expression:
V(1)@"MYFILE.DAT"
3
Click OK.
To identify the source file for an individual trace
1
In the trace legend, double-click the symbol for the trace
you want to identify (Figure 17-4).
trace symbols
Figure 17-4 Trace legend
symbols.
The Section Information dialog box appears, containing
the trace name and—if there is more than one waveform
data file loaded in the plot—the full path for the file from
which the trace was generated.
Also listed is information about the simulation that
generated the waveform data file and the number of data
points used (Figure 17-5).
Figure 17-5 Section information message box.
662
PSpice User's Guide
Product Version 10.5
Chapter overview
Saving simulation results in ASCII format
The default waveform data file format is binary. However, you
can save the waveform data file in the Common Simulation
Data Format (CSDF) instead.
Caution
Data files saved in the CSDF format are two or
more times the size of binary files.
When you first open a CSDF data file, PSpice converts it back
to the .DAT format. This conversion takes two or more times
as long as opening a .DAT file. PSpice saves the new .DAT file
for future use.
To save simulation results in ASCII format
PSpice User's Guide
1
From PSpice’s Simulation menu, choose Edit Profile to
display the Simulation Settings dialog box.
2
Click the Data Collection tab.
3
Select Save data in the CSDF format (.CSD).
4
Click OK.
663
Chapter 17
Analyzing waveforms
Product Version 10.5
PSpice writes simulation results to the waveform data file
in ASCII format (as *.CSD instead of *.DAT), following the
CSDF convention.
664
PSpice User's Guide
Product Version 10.5
Chapter overview
Analog example
In this section, basic techniques for performing waveform
analysis are demonstrated using the analog circuit
EXAMPLE.OPJ.
The example project EXAMPLE.OPJ is provided with your
installed programs. When shipped, EXAMPLE.OPJ is set up
with multiple analyses. For this example, the AC sweep, DC
sweep, Monte Carlo/worst-case, and small-signal transfer
function analyses have been disabled. The specification for
each of these disabled analyses remains intact. To run them
from Capture in the future, from the PSpice menu, choose Edit
Simulation Profile and enable the analyses.
Figure 17-6 Example schematic EXAMPLE.OPJ.
Running the simulation
The simulation is run with the Bias Point Detail, Temperature,
and Transient analyses enabled. The temperature analysis is
set to 35 degrees. The transient analysis is setup as follows:
Print Step
Final Time
Enable Fourier
PSpice User's Guide
20ns
1000ns
selected
665
Chapter 17
Analyzing waveforms
Product Version 10.5
Center Frequency
Output Vars
1Meg
V(OUT2)
Note: When you run a Fourier analysis using PSpice as
specified in this example, PSpice writes the results to
the PSpice output file (*.OUT). You can also use Probe
windows to display the Fourier transform of any trace
expression by using the FFT capability in PSpice. To
find out more, refer to the online PSpice Help.
To start the simulation
1
From Capture’s File menu, point to Open and choose
Project.
2
Open the following project in your installation directory:
\TOOLS\PSPICE\CAPTURE_SAMPLES\ANASIM\
EXAMPLE\EXAMPLE.OPJ
3
From the PSpice menu, choose Run to start the
simulation.
If PSpice is set to show traces for all markers on startup,
you will see the V(OUT1) and V(OUT2) traces when the
Probe window displays. To clear these traces from the
plot, from the Trace menu, choose Delete All Traces.
PSpice generates a binary waveform data file containing the
results of the simulation. A new Probe window appears with
666
PSpice User's Guide
Product Version 10.5
Chapter overview
the waveform data file EXAMPLE.DAT already loaded
(Figure 17-7).
Figure 17-7 Waveform display for EXAMPLE.DAT.
Because this sample project was set up as a transient
analysis type, the data currently loaded are the results of the
transient analysis.
Note: In this sample, the voltage markers for OUT1 and
OUT2 are already placed in the design. If the markers
are not placed prior to simulating, you can display the
waveforms later, as explained below in Displaying
voltages on nets.
Displaying voltages on nets
After selected an analysis, voltages on nets and currents into
device pins can be displayed in the Probe windows using
either schematic markers or output variables (as will be
demonstrated in this example).
PSpice User's Guide
667
Chapter 17
Analyzing waveforms
Product Version 10.5
To display the voltages at the OUT1 and OUT2 nets using
output variables
1
From the Trace menu, choose Add Trace to display the
Add Traces dialog box.
The Simulation Output Variables frame displays a list of
valid output variables.
2
668
Click V(OUT1) and V(OUT2), then click OK. The Probe
window should look similar to Figure 17-7.
PSpice User's Guide
Product Version 10.5
Chapter overview
Mixed analog/digital tutorial
In this tutorial, you will use PSpice A/D to simulate a simple,
mixed analog/digital circuit. You will then analyze the output
by:
■
simultaneously displaying analog and digital traces along
a common time axis, and
■
displaying digital data values and features unique to
mixed analog/digital circuit analysis, such as
identification of digital nets inserted by PSpice A/D.
About digital states
All digital states are supported in PSpice A/D. Logic levels
appear as shown below.
displays and prints red
displays and prints yellow
0
1
R
F
X
Nets with the Z strength (at any level) are displayed as a triple
line as shown below.
Z
displays and prints blue
PSpice User's Guide
669
Chapter 17
Analyzing waveforms
Product Version 10.5
About the oscillator circuit
The circuit you will simulate and analyze is a mixed
analog/digital oscillator using Schmitt trigger inverters, an
open-collector output inverter, a standard inverter, a JK
flip-flop, a resistor, and a capacitor. The design is shown in
Figure 17-8.
Figure 17-8 Mixed analog/digital oscillator
The circuit uses a one-bit digital stimulus device, DSTIM1. The
device is connected to the rest of the circuit by a single pin and
creates a reset pulse, which resets the flip-flop.
Setting up the design
Set up and simulate the oscillator circuit using Capture.
To open the design file
1
From Capture’s File menu, point to Open and choose
Project.
2
Open the following project in your OrCAD installation
directory:
\TOOLS\PSPICE\CAPTURE_SAMPLES\MIXSIM\OSC\
OSC.OPJ
To clear markers
1
670
From Capture’s PSpice menu, point to Markers and
choose Delete All.
PSpice User's Guide
Product Version 10.5
Chapter overview
Running the simulation
To run the simulation
1
From Capture’s PSpice menu, choose Edit Simulation
Profile and set the Run To Time to 5us.
2
From Capture’s PSpice menu, choose Run.
Because the oscillator circuit used here has been run with
only a transient analysis, PSpice automatically selects
the transient analysis data section from the waveform
data file. This means that the Available Selection dialog
box is skipped and a Probe window appears immediately.
Analyzing simulation results
To view the clock input to the inverter
1
From PSpice’s Trace menu, choose Add Trace to display
the Add Traces dialog box.
2
In the Simulation Output Variables list, click V(U3A:A) to
plot the input voltage to the inverter.
3
Click OK.
To add a second y-axis to avoid analog trace overlap
1
From the Plot menu, choose Axis Settings to display the
Axis Settings dialog box.
The X Axis tab is active by default.
Note: You can also open the X Axis tab in the Axis
Settings dialog box by double-clicking the x-axis in the
Probe window.
PSpice User's Guide
671
Chapter 17
Analyzing waveforms
Product Version 10.5
a. In the Data Range frame, choose User Defined and
set the range from 0us to 5us, if this is not already
set.
b. In the Scale frame, select Linear, if this is not already
set.
2
Click the Y Axis tab.
Note: You can also open the Y Axis tab in the Axis
Settings dialog box by double-clicking the y-axis in the
Probe window.
a. In the Data Range frame, choose User Defined and
set the range from -5 to 5. This will change the range
for the current y-axis.
b. Click OK.
Note: In the Y Axis Settings dialog box, you can change
the settings for another y-axis by selecting it from the Y
Axis Number box.
3
From the Plot menu, choose Add Y Axis.
The Probe window display should now look like
Figure 17-9 below.
Figure 17-9 Voltage at inverter input with y-axis
672
PSpice User's Guide
Product Version 10.5
Chapter overview
Note that the V(U3A:A) label at the bottom of the plot is
preceded by a boxed 1. This indicates that the far-left y-axis
applies to the V(U3A:A) waveform.
To view traces for V(CLK), RESET, and OUT
1
From the Trace menu, choose Add Trace to display the
Add Traces dialog box.
2
In the Simulation Output Variables list, click V(U1A:CLK),
RESET, and OUT.
The trace names appear in the Trace Expression text box.
Note: You can add up to 75 digital traces to the digital
portion of the plot. If you add more traces than can be
displayed, PSpice A/D scrolls the traces upwards so you
can see the last trace added. A + character in front of
the highest or lowest trace name indicates that there are
more traces above or below the marked traces.
3
Click OK to plot the traces.
The plot displays a digital area above the analog area as
shown in Figure 17-10 below.
Figure 17-10 Mixed analog/digital oscillator results.
PSpice User's Guide
673
Chapter 17
Analyzing waveforms
Product Version 10.5
User interface features for waveform analysis
PSpice provides direct manipulation techniques and shortcuts
for analyzing waveform data. These techniques are described
below.
Many of the menu commands in PSpice have equivalent
keyboard shortcuts. For instance, after placing a selection
rectangle in the analog portion of the plot, you can type Ctrl+A
instead of choosing Area from the View menu. For a list of
shortcut keys, see the online PSpice Help.
Zoom regions
PSpice provides a direct manipulation method for marking the
zoom region in either the digital or the analog area of the plot.
To zoom in or out
1
Do one of the following on the toolbar:
❑
Click the View In toolbar button
to zoom in by a
factor of 2 around the point you specify.
❑
Click the View Out toolbar button
to zoom out by
a factor of 2 around the point you specify.
To zoom in the digital area using the mouse
1
In the digital area, drag the mouse pointer left or right to
produce two vertical bars.
Note: Click the mouse anywhere on the plot to remove
the vertical bars without zooming.
zoom bars (digital)
674
PSpice User's Guide
Product Version 10.5
Chapter overview
2
From the View menu, point to Zoom, then choose Area.
PSpice changes the plot display to the area in between
the selection bars. If the plot includes an analog area, it is
zoomed in as well.
To zoom in the analog area using the mouse
1
Drag the mouse pointer to make a selection rectangle as
shown below.
Note: Click anywhere on the plot to remove the selection
rectangle without zooming.
selection rectangle (analog)
2
From the View menu, point to Zoom, then choose Area.
PSpice changes the plot to display the region within the
selection rectangle. The digital portion of the display, if
present, is also zoomed.
PSpice User's Guide
675
Chapter 17
Analyzing waveforms
Product Version 10.5
Scrolling traces
By default, when a plot is zoomed or when a digital plot
contains more traces than can be displayed in the visible area,
standard scroll bars appear to the right or at the bottom of the
plot area as necessary. These can be used to pan through the
data. You can configure scroll bars so they are always present
or are never displayed.
To configure scroll bars
1
In PSpice, from the Tools menu, choose Options.
2
In the Use Scroll Bars frame, choose one of the scroll
bars options, as described below.
Choose this
option...
To do this...
Auto
Have scroll bars appear when a plot is
zoomed or when additional traces are
displayed in the plot but are not visible
(default).
Never
Never display scroll bars. This mode
provides maximum plot size and is useful
on VGA and other low resolution displays.
Always
Display scroll bars at all times. However,
they are disabled if the corresponding axis
is full scale.
Sizing digital plots
Sizing bars can be used to change the digital plot size instead
of choosing Digital Size from the Plot menu. The digital trace
name sizing bar is at the left vertical boundary of the digital
plot. If an analog plot area is displayed simultaneously with the
digital plot, there is an additional plot sizing bar at the bottom
horizontal boundary of the digital plot.
676
PSpice User's Guide
Product Version 10.5
Chapter overview
To set the digital plot size using the mouse
1
Display at least one digital trace and one analog trace in
the Probe window for which you want to set the digital
size.
2
To change the bottom position of the digital Probe
window, do the following:
a. Place the mouse pointer between the analog and
digital parts of the plot.
b. Click the plot separator.
c. Drag the plot separator until you have the digital size
you want.
3
To change the left side of the digital Probe window, do the
following:
a. Place the mouse pointer at the left edge of the digital
Probe window you want to resize.
b. Click the left edge.
c. Drag the left edge of the digital Probe window to
adjust the space available for displaying digital trace
names.
To set the digital plot size using menu options
1
Display at least one digital trace in the plot for which you
want to set the digital size.
2
From the Plot menu, choose Digital Size.
3
In the Digital Size dialog box, set the following:
4
PSpice User's Guide
❑
Percentage of Plot to be Digital
❑
Length of Digital Trace Name
Click OK.
677
Chapter 17
Analyzing waveforms
Product Version 10.5
Modifying trace expressions and labels
You can modify trace expressions, text labels, and ellipse
labels that are currently displayed within the Probe window,
thus eliminating the need to delete and recreate any of these
objects.
1
To place a label, click Plot, point to Label and then choose
the desired type of object you want to place.
For information about adding labels (including text, line,
poly-line, arrow, box, circle, ellipse, and mark), refer to the
online PSpice Help.
To modify trace expressions
1
Click the trace name to select it (selection is indicated by
a color change).
2
From the Edit menu, choose Modify Object.
Note: You can also double-click the trace name to modify
the trace expression.
3
In the Modify Trace dialog box, edit the trace expression
just as you would when adding a trace.
For more information on adding traces, see Adding traces
from specific loaded waveform data files on page 661 and
To add traces using output variables on page 690.
To modify text and ellipse labels
1
Click the text or ellipse to select it (selection is indicated
by a color change).
2
From the Edit menu, choose Modify Object.
Note: You can also double-click a text or ellipse label to
modify it.
3
Edit the label by doing one of the following:
❑
678
In the Ellipse Label dialog box, change the inclination
angle.
PSpice User's Guide
Product Version 10.5
Chapter overview
❑
In the Text Label dialog box, change the text label.
Moving and copying trace names and expressions
Trace names and expressions can be selected and moved or
copied, either within the same Probe window or to another
Probe window.
To copy or move trace names and expressions
1
Click one or more (Shift+click) trace names. Selected
trace names are highlighted.
2
From the Edit menu, choose Copy or Cut to save the trace
names and expressions to the clipboard. Cut removes
trace names and traces from the Probe window.
3
In the Probe window where traces are to be added, do
one of the following:
4
❑
To add trace names to the end of the currently
displayed set, choose Paste from the Edit menu.
❑
To add traces before a currently displayed trace
name, select the trace name and then choose Paste
from the Edit menu.
Click OK.
Tip
When adding a trace to a Probe window, you can
make the trace display name different from the trace
expression:
a. From the Trace menu, choose Add Trace.
b. In the Trace Expression text box, enter a trace
expression using the syntax:
trace_expression[;display_name]
Here are some considerations when copying or moving trace
names and expressions into a different Probe window:
PSpice User's Guide
679
Chapter 17
Analyzing waveforms
Product Version 10.5
■
If the new Probe window is reading the same waveform
data file, the copied or moved trace names and
expressions display traces that are identical to the
original selection set.
■
If the new Probe window is reading a different waveform
data file, the copied or moved names and expressions
display different traces generated from the new data.
For example, suppose two waveform data files,
MYSIM.DAT and YOURSIM.DAT each contain a V(2)
waveform. Suppose also that two Probe windows are
currently displayed where window A is loaded with
MYSIM.DAT, and window B is loaded with YOURSIM.DAT.
When V(2) is copied from window A to window B, the
trace looks different because it is determined by data
from YOURSIM.DAT instead of MYSIM.DAT.
Copying and moving labels
Labels can be selected and moved or copied, either within the
same Probe window or to another Probe window.
For information about adding labels (including text, line,
poly-line, arrow, box, circle, ellipse, and mark), refer to the
online PSpice Help.
To copy labels
1
Select one or more (Shift+click) labels, or select multiple
labels by drawing a selection rectangle. Selected labels
are highlighted.
2
From the Edit menu, choose Copy or Cut to save the
labels to the clipboard.
Cut removes labels from the Probe window.
680
3
Switch to the Probe window where labels are to be
added, and from the Edit menu, choose Paste.
4
Click on the new location to place the labels.
PSpice User's Guide
Product Version 10.5
Chapter overview
To move labels
1
Select one or more (Shift+click) labels, or select multiple
labels by drawing a selection rectangle. Selected labels
are highlighted.
2
Move the labels by dragging them to a new location.
Tabulating trace data values
You can generate a table of data points reflecting one or more
traces in the Probe window and use this information in a
document or spreadsheet.
To view the trace data values table
1
Select one or more (Shift+click) trace names. Selected
trace names are highlighted.
2
From the Edit menu, choose Copy or Cut to save the trace
data point values to the Clipboard.
Cut removes traces from the Probe window.
3
In Clipboard Viewer, from the Display menu, choose
either Text or OEM Text.
To export the data points to other applications
1
Select one or more (Shift+click) trace names. Selected
trace names are highlighted.
2
From the Edit menu, choose Copy or Cut to save the trace
data point values to the Clipboard.
Cut removes traces from the Probe window.
3
Paste the data from the Clipboard into a text editor, a
spreadsheet program, or a technical computing program
(such as Mathcad).
4
Save the file.
Note: Saving the data directly to a file from Clipboard Viewer
can create superfluous data at the beginning of the file.
PSpice User's Guide
681
Chapter 17
Analyzing waveforms
Product Version 10.5
Using cursors
When one or more traces are displayed, you can use cursors
to display the exact coordinates of two points on the same
trace, or points on two different traces. In addition, differences
are shown between the corresponding coordinate values for
the two cursors.
Displaying cursors
To display both cursors
1
From the Trace menu, point to Cursor, then choose
Display.
The Probe Cursor window appears, showing the current
position of the cursor on the x-axis and y-axis. As you
move the cursors, the values in the cursor box change.
You can move the cursor box anywhere over the Probe
window by dragging the box to another location.
In the analog area of the plot (if any), both cursors are
initially placed on the trace listed first in the trace legend.
The corresponding trace symbol is outlined with a dashed
line.
In the digital area of the plot (if any), both cursors are
initially placed on the trace named first along the y-axis.
The corresponding trace name is outlined with a dashed
line.
Moving cursors
To move cursors along a trace using menu commands
1
From the Trace menu, point to Cursor, then choose Peak,
Trough, Slope, Min, Max, Point, or Search.
For more information about the cursor commands, refer to the
online PSpice Help.
682
PSpice User's Guide
Product Version 10.5
Chapter overview
To move cursors along a trace using the mouse
1
Use the right and left mouse buttons as described in
Table 17-8 below.
Table 17-8 Mouse actions for cursor control
Click this...
To do this with the cursors...
cursor assignment
Left-click the analog trace Associate the first cursor with
symbol or digital trace
the selected trace.
name.
Right-click the analog
trace symbol or digital
trace name.
Associate the second cursor
with the selected trace.
cursor movement
Left-click in the display
area.
Move the first cursor to the
closest trace segment at the
X position.
Right-click in the display
area.
Move the second cursor to the
closest trace segment at the
X position.
Note: For a family of curves (such as from a nested DC
sweep), you can use the mouse or the arrow keys to
move the cursor to one of the other curves in the family.
You can also click the desired curve.
To move cursors along a trace using the keyboard
1
Use key combinations as described in Table 17-9 below.
Table 17-9 Key combinations for cursor control
PSpice User's Guide
Us this key
combination...
To do this with the cursors...
Ctrl+Left arrow key and
Ctrl+Right arrow key
Change the trace associated
with the first cursor.
683
Chapter 17
Analyzing waveforms
Product Version 10.5
Table 17-9 Key combinations for cursor control,
Us this key
combination...
To do this with the cursors...
Shift+Ctrl+Left arrow key Change the trace associated
and Shift+Ctrl+Right
with the second cursor.
arrow key
Left arrow key and Right
arrow key
Move the first cursor along the
trace.
Shift+Left arrow key and Move the second cursor along
Shift+Right arrow key
the trace.
Home
Move the first cursor to the
beginning of the trace.
Shift+Home
Move the second cursor to the
beginning of the trace.
End
Move the first cursor to the end
of the trace.
Shift+End
Move the second cursor to the
end of the trace.
Applying cursors to a different trace
If you want to apply the cursors to a different trace, click the
trace symbol in the plot legend for the trace you want to
change to.
If you are displaying a large number of traces, and the symbol
is not shown for the trace you want to apply the cursors to, you
can apply the cursors to that trace in one of the following ways:
To apply the cursors to a different trace
1
Click in the cursor box to freeze the cursor locations on
the current trace.
2
After freezing the cursor locations, right-click on the new
trace you want to apply the cursors to.
- or -
684
PSpice User's Guide
Product Version 10.5
Chapter overview
1
From the Trace menu, choose Cursor, then choose
Freeze to freeze the cursor locations on the curren trace.
2
After freezing the cursor locations, right-click on the new
trace you want to apply the cursors to.
- or -
1
Press and hold the Shift key while right-clicking on the
new trace you want to apply the cursors to.
For more information about the cursor commands, refer to the
online PSpice Help.
Example: using cursors
Figure 17-11 shows both cursors positioned on the Out signal
in the digital area of a plot, and both cursors on the V(1)
waveform in the analog area of the plot.
digital
signal
w/cursors
cursor 1
results
cursor 2
results
analog
waveform
w/cursors
Figure 17-11 Cursors positioned on a trough and peak of
V(1)
Cursor 1 is positioned on the first trough (dip) of the V(1)
waveform. Cursor 2 is positioned on the second peak of the
same waveform.
Note: To position a cursor on the next trough of a waveform,
from the Trace menu, point to Cursor, then choose
Trough. To position a cursor on the next peak of a
PSpice User's Guide
685
Chapter 17
Analyzing waveforms
Product Version 10.5
waveform, from the Trace menu, point to Cursor, then
choose Peak.
In the Probe Cursor window, cursor 1 and cursor 2
coordinates are displayed (A1 and A2, respectively) with their
difference shown in the bottom line (dif). The logic state of the
Out signal is also displayed to the right of the cursor
coordinates.
The mouse buttons are also used to associate each cursor
with a different trace by clicking appropriately on either the
analog trace symbol in the legend or on the digital trace name
(see Table 17-8 on page 683). These are outlined in the
pattern corresponding to the associated cursor’s crosshair
pattern. Given the example in Figure 17-11, right-clicking the
V(2) symbol will associate cursor 2 with the V(2) waveform.
The analog legend now appears as shown below.
cursor 1
cursor 2
The Probe Cursor window also updates the A2 coordinates to
reflect the X and Y values corresponding to the V(2)
waveform.
For more information about cursors, refer to the online PSpice
Help.
686
PSpice User's Guide
Product Version 10.5
Chapter overview
Tracking digital simulation messages
PSpice A/D provides explanatory messages for errors that
occur during a digital simulation with their corresponding
waveforms. You can view messages from:
■
the Simulation Message Summary dialog box, or
■
the waveform display.
See Simulation condition messages on page 571 for
information on the message types that can be displayed by
PSpice A/D.
Message tracking from the message summary
A message summary is available for simulations where
diagnostics have been logged to the waveform data file. You
can display the message summary:
■
When loading a waveform data file (click OK when the
Simulation Errors dialog box appears).
■
Anytime by choosing Simulation Messages from the View
menu.
The Simulation Message Summary dialog box
The Simulation Message Summary dialog box lists message
header information.
You can filter the messages displayed in the list by selecting a
severity level from the Minimum Severity Level drop-down
menu. Messages are categorized (in decreasing order of
PSpice User's Guide
687
Chapter 17
Analyzing waveforms
Product Version 10.5
severity) as FATAL, SERIOUS, WARNING, or INFO
(informational).
When you select a severity level, the Message Summary
displays only those messages with the chosen severity or
higher. By default, the minimum severity level displayed is
SERIOUS.
Example: If you select WARNING as the minimum severity
level, the Simulation Message Summary dialog box will
display WARNING, SERIOUS, and FATAL messages.
To display waveforms associated with messages
1
In the Simulation Message Summary dialog box,
double-click a message.
For most message conditions, a Probe window appears
that contains the waveforms associated with the
simulation condition, along with detailed message text.
Persistent hazards
If a PERSISTENT HAZARD message is displayed, two plots
appear (see Figure 17-12), containing the following:
■
688
the waveforms that initially caused the timing violation or
hazard (lower plot)
PSpice User's Guide
Product Version 10.5
Trace expressions
■
the primary outputs or internal state devices to which the
condition has propagated (upper plot)
Figure 17-12 Waveform display for a persistent hazard.
Message tracking from the waveform
Trace segments with associated diagnostics are displayed in
the foreground color specified in your PSPICE.INI file. This
color is different from those used for standard state transitions.
To display explanatory message text
1
Double-click within the tagged region of a trace.
Trace expressions
Traces are referred to by output variable names. Output
variables are similar to the PSpice output variables specified
in the Simulation Settings dialog box for noise, Monte Carlo,
worst-case, transfer function, and Fourier analyses. However,
there are additional alias forms that are valid for trace
expressions. Both forms are discussed here.
PSpice User's Guide
689
Chapter 17
Analyzing waveforms
Product Version 10.5
To add traces using output variables
1
From the Trace menu, choose Add Trace to display the
Add Traces dialog box.
2
Construct a trace expression using any combination of
these controls:
❑
In the Simulation Output Variables frame, click output
variables.
You can display a subset of the available simulation
output variables by selecting or clearing the variable
type check boxes in the Simulation Output Variables
frame. Variable types not generated by the circuit
simulation are dimmed.
❑
In the Functions or Macros frame, select operators,
functions, constants, or macros.
❑
In the Trace Expression text box, type in or edit
output variables, operators, functions, constants, or
macros.
For more information about trace expressions, see
Analog trace expressions on page 700 and Digital
trace expressions on page 703.
3
If you want to change the name of the trace expression as
it displays in the Probe window, use the following syntax:
trace expression;display name
4
Click OK.
Basic output variable form
This form is representative of those used for specifying some
PSpice analyses.
690
PSpice User's Guide
Product Version 10.5
Trace expressions
<output>[AC suffix](<name>[,name])
Table 17-10
This placeholder...
Means this...
<output>
type of output quantity: V for voltage
or I for current (digital values do not
require a prefix)
[AC suffix]*
quantity to be reported for an AC
analysis. For a list of valid AC
suffixes, see Table 17-14 on
page 695
<name>[,name]
specifies either the net or
(+ net, - net) pair for which the
voltage is to be reported, or the
device for which a current is
reported, where:
■
net specifies either the net or
pin id (<fully qualified device
name>:<pin name>)
■
device name specifies the fully
qualified device name; for a list
of device types, see Table 17-15
on page 697 and Table 17-16
on page 697
A fully qualified device name
consists of the full hierarchical path
followed by the device’s reference
designator. For information about
the syntax for voltage output
variables, see Voltage on page 376.
PSpice User's Guide
691
Chapter 17
Analyzing waveforms
Product Version 10.5
Output variable form for device terminals
This form can only be specified for trace expressions. The
primary difference between this and the basic form is that the
terminal symbol appears before the net or device name
specification (whereas the basic form treats this as the pin
name within the pin id).
<output>[terminal]*[AC suffix](<name>[,name])
Table 17-11
This
placeholder...
Means this...
<output>
type of output quantity: V for voltage, I
for current, or N for noise (digital values
do not require a prefix)
[terminal]*
one or more terminals for devices with
more than two terminals; for a list of
terminal IDs, see Table 17-16 on
page 697
[AC suffix]*
quantity to be reported for an AC
analysis; for a list of valid AC suffixes,
see Table 17-14 on page 695
<name>[,<name> net, net pair, or fully qualified device
])
name; for a list of device types, see
Table 17-15 on page 697 and
Table 17-16 on page 697
Table 17-12 on page 693 summarizes the valid output
formats. Table 17-13 on page 695 provides examples of
692
PSpice User's Guide
Product Version 10.5
Trace expressions
equivalent output variables. Note that some of the output
variable formats are unique to trace expressions.
Table 17-12 Output variable formats
Format
Meaning
Voltage variables
V[ac](< +analog net > [,< -analog net Voltage between +
>])
and - analog net
ids
V<pin name>[ac](< device >)
Voltage at pin
name of a device
V< x >[ac](< 3 or 4-terminal device
>)
Voltage at
non-grounded
terminal x of a
3 or 4-terminal
device
V< z >[ac](< transmission line
device >)
Voltage at end z of
a transmission
line device (z is
either A or B)
Current variables
I[ac](< device >)
Current into a
device
I< x >[ac](< 3 or 4-terminal device >) Current into
terminal x of a
3 or 4-terminal
device
I< z >[ac](< transmission line device Current into end z
>)
of a transmission
line device (z is
either A or B)
Digital signal and bus variables
< digital net >[;< display name >]
PSpice User's Guide
Digital state at
digital net labeled
as display name
693
Chapter 17
Analyzing waveforms
Product Version 10.5
Table 17-12 Output variable formats, continued
Format
Meaning
{< digital net >*}[;< display name >]
[;< radix >]
Digital bus labeled
as display name
and of specified
radix
Sweep variables
< DC sweep variable >
name of any
variable used in
the DC sweep
analysis
FREQUENCY
AC analysis sweep
variable
TIME
transient analysis
sweep variable
Noise variables
V[db](ONOISE)
total
RMS-summed
noise at output net
V[db](INOISE)
total equivalent
noise at input
source
NTOT(ONOISE)
sum of all noise
contributors in the
circuit
N< noise type >(< device name >)
contribution from
noise type of
device name to
the total output
noise1
1. See Table 17-17 on page 698 for a complete list of noise types
by device type. For information about noise output variable
equations, the units used to represent noise quantities in trace
expressions, and a noise analysis example, see Analyzing
Noise in the Probe window on page 452.
694
PSpice User's Guide
Product Version 10.5
Trace expressions
Table 17-13 Examples of output variable formats
A basic form
An alias
equivalent
Meaning
V(NET3,NET2) (same)
voltage between analog nets
labeled NET3 and NET2
V(C1:1)
V1(C1)
voltage at pin1 of capacitor
C1
VP(Q2:B)
VBP(Q2)
phase of voltage at base of
bipolar transistor Q2
V(T32:A)
VA(T32)
voltage at port A of
transmission line T32
I(M1:D)
ID(M1)
current through drain of
MOSFET device M1
QA
(same)
digital state at net QA
{IN1, IN2, IN3}; (same)
MYBUS;X
digital bus made of 3 digital
nets (IN1, IN2, IN3) named
MYBUS displayed in
hexadecimal
VIN
(same)
voltage source named VIN
FREQUENCY
(same)
AC analysis sweep variable
NFID(M1)
(same)
flicker noise from MOSFET
M1
Table 17-14 Output variable AC suffixes
PSpice User's Guide
Suffix
Meaning of output variables
none
magnitude
DB
magnitude in decibels
G
group delay (-dPHASE/dFREQUENCY)
I
imaginary part
M
magnitude
P
phase in degrees
695
Chapter 17
Analyzing waveforms
Product Version 10.5
Table 17-14 Output variable AC suffixes
696
Suffix
Meaning of output variables
R
real part
PSpice User's Guide
Product Version 10.5
Trace expressions
Table 17-15 Device names for two-terminal device types
Two-terminal device type1
Device type letter
capacitor
C
diode
D
voltage-controlled voltage source2 E
current-controlled current source2 F
voltage-controlled current source2 G
current-controlled voltage source2 H
independent current source
I
inductor
L
resistor
R
voltage-controlled switch2
S
independent voltage source
V
current-controlled switch2
W
1. The pin name for two-terminal devices is either 1 or 2.
2. The controlling inputs for these devices are not considered
terminals.
Table 17-16 Terminal IDs by three & four-terminal device
type
Three & four-terminal
device type
Device type
letter
Terminal IDs
GaAs MOSFET
B
D (drain)
G (gate)
S (source)
Junction FET
J
D (drain)
G (gate)
S (source)
PSpice User's Guide
697
Chapter 17
Analyzing waveforms
Product Version 10.5
Table 17-16 Terminal IDs by three & four-terminal device
type
Three & four-terminal
device type
Device type
letter
Terminal IDs
MOSFET
M
D (drain)
G (gate)
S (source)
B (bulk, substrate)
Bipolar transistor
Q
C (collector)
B (base)
E (emitter)
S (substrate)
transmission line
T
A (near side)
B (far side)
IGBT
Z
C (collector)
G (gate)
E (emitter)
Table 17-17 Noise types by device type
Device type
Noise
types1
Meaning
B (GaAsFET)
FID
RD
RG
RS
SID
TOT
flicker noise
thermal noise associated with RD
thermal noise associated with RG
thermal noise associated with RS
shot noise
total noise
D (diode)
FID
RS
SID
TOT
flicker noise
thermal noise associated with RS
shot noise
total noise
698
PSpice User's Guide
Product Version 10.5
Trace expressions
Table 17-17 Noise types by device type
Digital Input
RHI
RLO
TOT
thermal noise associated with RHI
thermal noise associated with RLO
total noise
Digital Output
TOT
total noise
J (JFET)
FID
RD
RG
RS
SID
TOT
flicker noise
thermal noise associated with RD
thermal noise associated with RG
thermal noise associated with RS
shot noise
total noise
M (MOSFET)
FID
RB
RD
RG
RS
SID
TOT
flicker noise
thermal noise associated with RB
thermal noise associated with RD
thermal noise associated with RG
thermal noise associated with RS
shot noise
total noise
Q (BJT)
FIB
RB
RC
RE
SIB
SIC
TOT
flicker noise
thermal noise associated with RB
thermal noise associated with RC
thermal noise associated with RE
shot noise associated with base current
shot noise associated with collector current
total noise
R (resistor)
TOT
total noise
Iswitch
TOT
total noise
Vswitch
TOT
total noise
1. These variables report the contribution of the specified device’s noise to the total output noise in
units of V2/Hz. This means that the sum of all device noise contributions is equal to the total output
noise in V2/Hz, NTOT(ONOISE).
PSpice User's Guide
699
Chapter 17
Analyzing waveforms
Product Version 10.5
Analog trace expressions
Trace expression aliases
Analog trace expressions vary from the output variables used
in simulation analyses because analog net values can be
specified by:
<output variable>[;display name]
as opposed to the <output variable> format used in
analyses. With this format, the analog trace expression can be
displayed in the analog legend with an optional alias.
Arithmetic functions
Arithmetic expressions of analog output variables use the
same operators as those used in simulation analyses (by
means of part property definitions in Capture). You can also
include intrinsic functions in expressions. The intrinsic
functions available for trace expressions are similar to those
available for PSpice math expressions, but with some
differences, as shown in Table 17-18. A complete list of
PSpice arithmetic functions can be found in Table 3-4 on
page 126.
Table 17-18 Analog arithmetic functions for trace
expressions
700
Probe
function
Description
Available in
PSpice?
ABS(x)
|x|
YES
SGN(x)
+1 (if x>0), 0 (if x=0), -1 (if
x<0)
YES
SQRT(x)
x1/2
YES
EXP(x)
ex
YES
LOG(x)
ln(x)
YES
LOG10(x)
log(x)
YES
M(x)
magnitude of x
YES
PSpice User's Guide
Product Version 10.5
Trace expressions
Table 17-18 Analog arithmetic functions for trace
expressions, continued
Probe
function
Description
Available in
PSpice?
P(x)
phase of x (degrees)
YES
R(x)
real part of x
YES
IMG(x)
imaginary part of x
YES
G(x)
group delay of x (seconds)
NO
PWR(x,y)
|x|y
YES
SIN(x)
sin(x)
YES
COS(x)
cos(x)
YES
TAN(x)
tan(x)
YES
ATAN(x)
tan -1 (x)
ARCTAN(x
)
PSpice User's Guide
YES
d(x)
derivative of x with respect to YES1
the x-axis variable
s(x)
integral of x over the range of YES2
the x-axis variable
AVG(x)
running average of x over the NO
range of the x-axis variable
AVGX(x,d) running average of x from
X_axis_value(x)-d to
X_axis_value(x)
NO
RMS(x)
running RMS average of x
over the range of the x-axis
variable
NO
DB(x)
magnitude in decibels of x
NO
MIN(x)
minimum of the real part of x NO
MAX(x)
maximum of the real part of x NO
701
Chapter 17
Analyzing waveforms
Product Version 10.5
Table 17-18 Analog arithmetic functions for trace
expressions, continued
Probe
function
Description
Available in
PSpice?
ENVMIN(x, Envelope of x.Valley lows
d)
selected have a minimum
number of d consecutive
datapoints.
NO
ENVMAX(x Envelope of x. Peaks
,d)
selected have a minimum
number of d consecutive
datapoints.
NO
1. In PSpice, this function is called DDT(x).
2. In PSpice, this function is called SDT(x).
Note: For AC analysis, PSpice uses complex arithmetic to
evaluate trace expressions. If the result of the
expression is complex, then its magnitude is displayed.
Rules for numeric values suffixes
Explicit numeric values are entered in trace expressions in the
same form as in simulation analyses (by means of part
properties in Capture), with the following exceptions:
■
Suffixes M and MEG are replaced with m (milli, 1E-3) and
M (mega, 1E+6), respectively.
■
MIL and mil are not supported.
■
With the exception of the m and M scale suffixes, PSpice
is not case sensitive; therefore, upper and lower case
characters are equivalent.
Example: V(5) and v(5) are equivalent in trace
expressions.
Unit suffixes are only used to label the axis; they never affect
the numerical results. Therefore, it is always safe to leave off
a unit suffix.
702
PSpice User's Guide
Product Version 10.5
Trace expressions
Example: The quantities 2e-3, 2mV, and .002v all have the
same numerical value. For axis labeling purposes, PSpice
recognizes that the second and third forms are in volts,
whereas the first is dimensionless.
PSpice also knows that W=V·A, V=W/A, and A=W/V. So, if you
add this trace:
V(5)*ID(M13)
the axis values are labeled with W.
For a demonstration of analog trace presentation, see Analog
example on page 665
The units to use for trace expressions are shown in Table
17-19.
Table 17-19 Output units for trace expressions
Symbol
Unit
V
volt
A
amps
W
watt
d
degree (of phase)
s
second
Hz
hertz
Digital trace expressions
Digital output variables in trace expressions vary from those
used in simulation analyses as follows:
■
Digital net values are specified by:
<digital net>[;display name]
as opposed to the <digital net> format used for
analyses. With this format, the digital signal can be
displayed on the digital plot with an optional alias.
PSpice User's Guide
703
Chapter 17
Analyzing waveforms
Product Version 10.5
■
The output from several digital nets can be collected into
a single output of higher radix known as a bus.
Example: You can request that four bus lines be displayed
together as one hexadecimal digit. You can combine up
to 32 digital signals into a bus.
A bus is formed by enclosing a list of digital net names
(separated by blanks or commas) within braces
according to the format:
{<high-order net> [mid-order net]* <low-order
net>}
The elements of the bus definition, taken left to right,
specify the output values of the bus from high order to low
order.
Example: { Q2, Q1, Q0 } specifies a 3-bit bus whose
high-order bit is the digital value at net Q2.
By definition, a digital signal is any digital net value or a
logical expression involving digital nets. For the digital output
variable formats described earlier, you can use a digital signal
expression everywhere a net name is expected. You can also
form buses into expressions using both logical and arithmetic
operators.
As a result, the generalized form for defining a digital trace is:
<digital trace expression> [;display name [;radix]]
Exception: You can display your radix designation option with
the digital trace expression by leaving the display name blank
and using the following syntax:
digital trace expression;;radix
Table 17-20
704
This
placeholder...
Means this...
digital trace
expression
expression of digital buses or
digital signals.
PSpice User's Guide
Product Version 10.5
Trace expressions
Table 17-20
This
placeholder...
Means this...
display name
name that will be displayed on the
screen; if no display name is
specified, the actual trace
expression is used; if a display
name is given, it is available for
use in subsequent trace
definitions.
radix
applies only to bus expressions
and denotes the radix in which
the bus value is to be displayed;
the radix is specified as:
H or X
D
O
B
hexadecimal (default)
decimal
octal
binary
Table 17-21 presents the operators available for digital signal
and bus expressions listed in order of precedence (high to
low).
Table 17-21 Digital logical and arithmetic operators
PSpice User's Guide
Operator
Meaning
()
grouping
~
logical complement
*
multiplication (bus values only)
/
division (bus values only)
+
addition (bus values only)
-
subtraction (bus values only)
&
and
^
exclusive or
|
or
705
Chapter 17
Analyzing waveforms
Product Version 10.5
An arithmetic or logical operation between two bus operands
results in a bus value that is as wide as is necessary to contain
the result. Prior to the operation, if necessary, the shorter
operand is extended to the width of the longer operand by
zero-filling on the high-order end.
An arithmetic or logical operation between a bus operand and
a signal operand results in a bus value. Prior to the operation,
the signal is converted to a bus of width one, then extended if
necessary.
You can use signal constants in signal expressions. Specify
them as shown in Table 17-22.
Table 17-22 Signal constants for digital trace
expressions
Signal
Constant
Meaning
’0
low
’1
high
’F
falling
’R
rising
’X
unknown
’Z
high impedance
You can use bus constants in bus expressions. Specify them
as strings of the form:
706
PSpice User's Guide
Product Version 10.5
Trace expressions
r'ddd
Table 17-23
This
placeholder...
Means this...
r
case-insensitive radix specifier (x,
h, d, o, or b)
ddd
string of digits appropriate to the
specified radix
Table 17-24 Example notations for bus constants:
This notation...
Has this radix...
x'3FFFF
hexadecimal
h'5a
hexadecimal
d'79
decimal
o'177400
octal
b'100110
binary
For a procedural discussion of digital trace expressions, see
Analyzing results on page 563 in the Digital simulation
chapter.
For a discussion and demonstration of digital trace
presentation, complete the Mixed analog/digital tutorial on
page 669.
PSpice User's Guide
707
Chapter 17
708
Analyzing waveforms
Product Version 10.5
PSpice User's Guide
Measurement expressions
18
Chapter overview
This chapter describes how to put together measurement
expressions using the measurement definitions included with
PSpice. The Power Users section includes instructions on
how to compose your own measurement definitions.
■
Measurements overview on page 710
■
Measurement strategy on page 711
■
Procedure for creating measurement expressions on
page 712
■
Example on page 714
■
PSpice User's Guide
For power users on page 721
709
Chapter 18
Measurement expressions
Product Version 10.5
Measurements overview
Measurement expressions evaluate the characteristics of a
waveform. A measurement expression is made by choosing
the waveform and the waveform calculation you want to
evaluate.
The waveform calculation is defined by a measurement
definition such as rise time, bandpass bandwidth, minimum
value, and maximum value.
For example, if you want to measure the risetime of your circuit
output voltage, use the following expression:
Risetime(v(out))
For a list of the PSpice measurement definitions, see
Measurement definitions included in PSpice on page 718.
You can also create your own custom measurement
definitions. See Creating custom measurement definitions on
page 721 in the Power Users section of this chapter.
710
PSpice User's Guide
Product Version 10.5
Chapter overview
Measurement strategy
PSpice User's Guide
■
Start with a circuit created in Capture and a working
PSpice simulation.
■
Decide what you want to measure.
■
Select the measurement definition that matches the
waveform characteristics you want to measure.
■
Insert the output variable (whose waveform you want to
measure) into the measurement definition, to form a
measurement expression.
■
Test the measurement expression.
711
Chapter 18
Measurement expressions
Product Version 10.5
Procedure for creating measurement expressions
Setup
Before you create a measurement expression:
1
Design a circuit in Capture.
2
Set up a PSpice simulation:
3
❑
Time Domain (transient)
❑
DC Sweep
❑
AC Sweep/Noise
Run the circuit in PSpice.
Make sure the circuit is valid and you have the results you
expect.
Composing a measurement expression
These steps show you how to create a measurement
expression in PSpice.
First select a measurement definition, and then select output
variables to measure. The two combined become a
measurement expression.
Work in the Simulation Results view in PSpice. In the side
toolbar, click on
.
1
From the Trace menu in PSpice, select Measurements.
The Measurements dialog box appears.
2
Select the measurement definition you want to evaluate.
3
Click Eval (evaluate).
The Arguments for Measurement Evaluation dialog
box appears.
4
712
Click the Name of trace to search button.
PSpice User's Guide
Product Version 10.5
Chapter overview
The Traces for Measurement Arguments dialog box
appears.
Note: You will only be using the Simulation Output
Variables list on the left side. Ignore the Functions or
Macros list.
5
Uncheck the output types you don’t need (if you want to
simplify the list).
6
Click on the output variable you want to evaluate.
The output variable appears in the Trace Expression
field.
7
Click OK.
The Arguments for Measurement Evaluation dialog
box reappears with the output variable you chose in the
Name of trace to search field.
8
Click OK.
Your new measurement expression is evaluated and
displayed in the PSpice window.
9
Click OK in the Display Measurement Evaluation
pop-up box to continue working in PSpice.
Your new measurement expression is saved, but it no
longer displays in the window. The only way to get
another graphical display is to redo these steps.
You can see a numerical evaluation by following the next
steps.
Viewing the results of measurement evaluations
1
From the View menu in PSpice, select Measurement
Results.
The Measurement Results table displays below the plot
window.
2
Click the box in the Evaluate column.
The PSpice calculation for your measurement expression
appears in the Value column.
PSpice User's Guide
713
Chapter 18
Measurement expressions
Product Version 10.5
Example
First you select a measurement definition, and then you select
an output variable to measure. The two combined become a
measurement expression.
Work in the Simulation Results view in PSpice. In the side
toolbar, click on
.
1
From the Trace menu in PSpice, select Measurements.
The Measurements dialog box appears.
2
Select the measurement definition you want to evaluate.
3
Click Eval (evaluate).
The Arguments for Measurement Evaluation dialog
box appears.
4
714
Click the Name of trace to search button.
PSpice User's Guide
Product Version 10.5
Chapter overview
The Traces for Measurement Arguments dialog box
appears.
Note: You will only be using the Simulation Output
Variables list on the left side. Ignore the Functions or
Macros list.
PSpice User's Guide
715
Chapter 18
Measurement expressions
Product Version 10.5
5
Uncheck the output types you don’t need (if you want to
simplify the list).
6
Click on the output variable you want to evaluate.
The output variable appears in the Trace Expression
field.
7
Click OK.
The Arguments for Measurement Evaluation dialog
box reappears with the output variable you chose in the
Name of trace to search field.
8
Click OK.
Your new measurement expression is evaluated and
displayed in the PSpice window.
716
PSpice User's Guide
Product Version 10.5
Chapter overview
9
Click OK in the Display Measurement Evaluation
pop-up box to continue working in PSpice.
Your new measurement expression is saved, but does not
display in the window. The only way to get another
graphical display is to redo these steps. You can see a
numerical evaluation by following the next steps.
10 Click Close.
Viewing the results of measurement evaluations.
1
From the View menu, select Measurement Results.
The Measurement Results table displays below the plot
window.
2
Click the box in the Evaluate column.
A check mark appears in the Evaluate column check box
and the PSpice calculation for your measurement
expression appears in the Value column.
PSpice User's Guide
717
Chapter 18
Measurement expressions
Product Version 10.5
Measurement definitions included in PSpice
Definition
Finds the. . .
Bandwidth
Bandwidth of a waveform (you choose dB level)
Bandwidth_Bandpass_3dB
Bandwidth (3dB level) of a waveform
Bandwidth_Bandpass_3dB_XRange Bandwidth (3dB level) of a waveform over a
specified X-range
CenterFrequency
Center frequency (dB level) of a waveform
CenterFrequency_XRange
Center frequency (dB level) of a waveform over a
specified X-range
ConversionGain
Ratio of the maximum value of the first waveform to
the maximum value of the second waveform
ConversionGain_XRange
Ratio of the maximum value of the first waveform to
the maximum value of the second waveform over a
specified X-range
Cutoff_Highpass_3dB
High pass bandwidth (for the given dB level)
Cutoff_Highpass_3dB_XRange
High pass bandwidth (for the given dB level)
Cutoff_Lowpass_3dB
Low pass bandwidth (for the given dB level)
Cutoff_Lowpass_3dB_XRange
Low pass bandwidth (for the given dB level) over a
specified range
DutyCycle
Duty cycle of the first pulse/period
DutyCycle_XRange
Duty cycle of the first pulse/period over a range
Falltime_NoOvershoot
Falltime with no overshoot.
Falltime_StepResponse
Falltime of a negative-going step response curve
Falltime_StepResponse_XRange
Falltime of a negative-going step response curve
over a specified range
GainMargin
Gain (dB level) at the first 180-degree out-of-phase
mark
Max
Maximum value of the waveform
Max_XRange
Maximum value of the waveform within the
specified range of X
Min
Minimum value of the waveform
718
PSpice User's Guide
Product Version 10.5
Chapter overview
Definition
Finds the. . .
Min_XRange
Minimum value of the waveform within the
specified range of X
NthPeak
Value of a waveform at its nth peak
Overshoot
Overshoot of a step response curve
Overshoot_XRange
Overshoot of a step response curve over a
specified range
Peak
Value of a waveform at its nth peak
Period
Period of a time domain signal
Period_XRange
Period of a time domain signal over a specified
range
PhaseMargin
Phase margin
PowerDissipation_mW
Total power dissipation in milli-watts during the
final period of time (can be used to calculate total
power dissipation, if the first waveform is the
integral of V(load)
Pulsewidth
Width of the first pulse
Pulsewidth_XRange
Width of the first pulse at a specified range
Q_Bandpass
Calculates Q (center frequency / bandwidth) of a
bandpass response at the specified dB point
Q_Bandpass_XRange
Calculates Q (center frequency / bandwidth) of a
bandpass response at the specified dB point and
the specified range
Risetime_NoOvershoot
Risetime of a step response curve with no
overshoot
Risetime_StepResponse
Risetime of a step response curve
Risetime_StepResponse_XRange
Risetime of a step response curve at a specified
range
SettlingTime
Time from <begin_x> to the time it takes a step
response to settle within a specified band
SettlingTime_XRange
Time from <begin_x> to the time it takes a step
response to settle within a specified band and
within a specified range
PSpice User's Guide
719
Chapter 18
Measurement expressions
Product Version 10.5
Definition
Finds the. . .
SlewRate_Fall
Slew rate of a negative-going step response curve
SlewRate_Fall_XRange
Slew rate of a negative-going step response curve
over an X-range
SlewRate_Rise
Slew rate of a positive-going step response curve
SlewRate_Rise_XRange
Slew rate of a positive-going step response curve
over an X-range
Swing_XRange
Difference between the maximum and minimum
values of the waveform within the specified range
XatNthY
Value of X corresponding to the nth occurrence of
the given Y_value, for the specified waveform
XatNthY_NegativeSlope
Value of X corresponding to the nth negative slope
crossing of the given Y_value, for the specified
waveform
XatNthY_PercentYRange
Value of X corresponding to the nth occurrence of
the waveform crossing the given percentage of its
full Y-axis range; specifically, nth occurrence of
Y=Ymin+(Ymax-Ymin)*Y_pct/100
XatNthY_Positive Slope
Value of X corresponding to the nth positive slope
crossing of the given Y_value, for the specified
waveform
YatFirstX
Value of the waveform at the beginning of the
X_value range
YatLastX
Value of the waveform at the end of the X_value
range
YatX
Value of the waveform at the given X_value
YatX_PercentXRange
Value of the waveform at the given percentage of
the X-axis range
ZeroCross
X-value where the Y-value first crosses zero
ZeroCross_XRange
X-value where the Y-value first crosses zero at the
specified range
720
PSpice User's Guide
Product Version 10.5
For power users
For power users
Creating custom measurement definitions
Measurement definitions establish rules to locate interesting
points and compute values for a waveform. In order to do this,
a measurement definition needs:
■
A measurement definition name
■
A marked point expression
These are the calculations that compute the final point on
the waveform.
■
One or more search commands
These commands specify how to search for the
interesting points.
Strategy
1
Decide what you want to measure.
2
Examine the waveforms you have and choose which
points on the waveform are needed to calculate the
measured value.
3
Compose the search commands to find and mark the
desired points.
4
Use the marked points in the Marked Point Expressions
to calculate the final value for the waveform.
5
Test the search commands and measurements.
Note: An easy way to create a new definition:
From the PSpice Trace menu, select Measurements to
open the Measurements dialog box, then:
PSpice User's Guide
❍
Select the definition most similar to your needs
❍
Click Copy and follow the prompts to rename
and edit.
721
Chapter 18
Measurement expressions
Product Version 10.5
Writing a new measurement definition
1
From the PSpice Trace menu, choose Measurements.
The Measurements dialog box appears.
2
Click New.
The New Measurement dialog box appears.
3
Type a name for the new measurement in the New
Measurement name field.
Make sure local file is selected.
This stores the new measurement in a .prb file local to the
design.
4
Click OK.
The Edit New Measurement dialog box appears.
5
Type in the marked expression.
6
Type in any comments you want.
7
Type in the search function.
Note: For syntax information, see Measurement definition
syntax on page 725
Your new measurement definition is now listed in the
Measurements dialog box.
Using the new measurement definition
Your new measurement definition is now listed in the
Measurements dialog box.
Note: For steps on using a definition in a measurement
expression to evaluate a trace, see Composing a
measurement expression on page 712.
Definition example
1
722
From the PSpice Trace menu, choose Measurements.
PSpice User's Guide
Product Version 10.5
For power users
The Measurements dialog box appears.
2
Click New.
The New Measurement dialog box appears.
3
Type in a name in the New Measurement name field.
4
Make sure use local file is selected.
This stores the new measurement in a .prb file local to the
design.
5
PSpice User's Guide
Click OK.
723
Chapter 18
Measurement expressions
Product Version 10.5
The Edit New Measurement dialog box appears.
marked point
expression
comments
search function
6
Type in the marked expression:
point707(1) = y1
7
Type in the search function.
{
1|Search forward level(70.7%, p) !1;
}
Note: The search function is enclosed within curly
braces.
Always place a semicolon at the end of the last search
function.
8
Type in any explanatory comments you want:
*
*#Desc#* Find the .707 value of the trace.
*
*#Arg1#* Name of trace to search
*
Note: For syntax information, see Measurement definition
syntax on page 725.
Using the new measurement definition
Your new measurement definition is now listed in the
Measurements dialog box.
724
PSpice User's Guide
Product Version 10.5
For power users
For an example of using a definition in a measurement
expression to evaluate a trace, see Example on page 714.
Measurement definition syntax
Check out the existing measurement definitions in PSpice for
syntax examples.
1
From the Trace menu in PSpice, choose
Measurements.
The Measurement dialog box appears.
2
PSpice User's Guide
Highlight any example, and select View to examine the
syntax.
725
Chapter 18
Measurement expressions
Product Version 10.5
Measurement definition: fill in the place holders
measurement_name (1, [2, …, n][, subarg1, subarg2, …, subargm]) =
marked_point_expression
{
1| search_commands_and_marked_points_for_expression_1;
2| search_commands_and_marked_points_for_expression_2;
n| search_commands_and_marked_points_for_expression_n;
}
Measurement name syntax
Can contain any alphanumeric character (A-Z, 0-9) or
underscore _ , up to 50 characters in length. The first
character should be an upper or lower case letter.
Examples of valid function names: Bandwidth, CenterFreq,
delay_time, DBlevel1.
Comments syntax
A comment line always starts with an asterisk. Special
comment lines include the following examples:
*#Desc#*
The measurement description
*#Arg1#*
Description of an argument used in the measurement
definition.
726
PSpice User's Guide
Product Version 10.5
For power users
These comment lines will be used in dialog boxes, such as the
Arguments for Measurement Evaluation box.
Marked Point Expressions syntax
A marked point expression calculates a single value, which is
the value of the measurement, based on the X and Y
coordinates of one or more marked points on a curve. The
marked points are found by the search command.
All the arithmetic operators (+, -, *, /, ( ) ) and all the functions
that apply to a single point (for example, ABS(), SGN(), SIN(),
SQRT() ) can be used in marked point expressions.
The result of the expression is one number (a real value).
Marked point expressions differ from a regular expression in
the following ways:
PSpice User's Guide
■
Marked point coordinate values (for example, x1, y3), are
used instead of simulation output variables (v(4), ic(Q1)).
■
Multiple-point functions such as d(), s(), AVG(), RMS(),
MIN(), and MAX() cannot be used.
■
Complex functions such as M(), P(), R(), IMG(), and G()
cannot be used.
727
Chapter 18
Measurement expressions
■
Product Version 10.5
One additional function called MPAVG can also be used.
It is used to find the average Y value between 2 marked
points. The format is:
MPAVG(p1, p2,[<.fraction>])
where p1 and p2 are marked X points and fraction
(expressed in decimal form) specifies the range. The
range specified by [<.fraction>] is centered on the
midpoint of the total range. The default value is 1.
Example:
The marked point expression
MPAVG (x1, x5, .2)
will find the halfway point between x1 and x5 and will calculate
the average Y value based on the 20 percent of the range that
is centered on the halfway point.
Search command syntax
search [direction] [/start_point/] [#consecutive_points#] [(range_x [,range_y])]
[for]
[repeat:] <condition>
Brackets indicate optional arguments.
You can use uppercase or lowercase characters, because
searches are case independent.
[direction]
forward or backward
The direction of the search. Search commands can specify
either a forward or reverse direction. The search begins at the
origin of the curve.
[Forward] searches in the normal X expression direction,
which may appear as backwards on the plot if the X axis has
been reversed with a user-defined range.
728
PSpice User's Guide
Product Version 10.5
For power users
Forward is the default direction.
[/start_point/]
The starting point to begin a search. The current point is the
default.
Use this… To start the search at this…
^
the first point in the search range
Begin
the first point in the search range
$
the last point in the search range
End
the last point in the search range
xn
a marked point number
or an expression of marked points, for
example,
x1
(x1 - (x2 - x1) / 2)
[#consecutive points#]
Defines the number of consecutive points required for a
condition to be met. Usage varies for individual conditions; the
default is 1.
A peak is a data point with one neighboring data point on both
sides that has a lower Y value than the data point.
If [#consecutive_points#] is 2 and <condition> is PEak, then
the peak searched for is a data point with two neighboring
data points on both sides with lower Y values than the marked
data point.
[(range_x[,range_y])]
Specifies the range of values to confine the search.
The range can be specified as floating-point values, as a
percent of the full range, as marked points, or as an
expression of marked points. The default range is all points
available.
PSpice User's Guide
729
Chapter 18
Measurement expressions
Product Version 10.5
Examples
This range…
Means this…
(1n,200n)
X range limited from 1e-9 to 200e-9,
Y range defaults to full range
(1.5,20e-9,0,1m both X and Y ranges are limited
)
(5m,1,10%,90% both X and Y ranges are limited
)
(0%,100%,1,3)
full X range, limited Y range
(,,1,3)
full X range, limited Y range
(,30n)
X range limited only on upper end
[for] [repeat:]
Specifies which occurrence of <condition> to find.
If repeat is greater than the number of found instances of
<condition>, then the last <condition> found is used.
Example
The argument:
2:LEvel
would find the second level crossing.
<condition>
Must be exactly one of the following:
730
■
LEvel(value[,posneg])
■
SLope[(posneg)]
■
PEak
■
TRough
■
MAx
■
MIn
■
POint
PSpice User's Guide
Product Version 10.5
For power users
■
XValue(value)
Each <condition> requires just the first 2 characters of the
word. For example, you can shorten LEvel to LE.
If a <condition> is not found, then either the cursor is not
moved or the goal function is not evaluated.
LEvel(value[,posneg])
Finds the next Y value crossing at the specified level.
This can be between real data points, in which case an
interpolated artificial point is created.
[,posneg]
At least [#consecutive_points#]-1 points following the level
crossing point must be on the same side of the level crossing
for the first point to count as the level crossing.
[,posneg] can be Positive (P), Negative (P), or Both (B). The
default is Both.
(value)
can take any of the following forms:
Value form
Example
a floating number
1e5
100n
1
a percentage of full range 50%
a marked point
x1
y1
PSpice User's Guide
or an expression of
marked points
(x1-x2)/2
a value relative to
startvalue
.-3 ⇒ startvalue -3
a db value relative to
startvalue
.-3db ⇒ 3db below startvalue
a value relative to max or
min
max-3 ⇒ maxrng -3
.+3 ⇒ startvalue +3
.+3db ⇒ 3db above startvalue
min+3 ⇒ minrng +3
731
Chapter 18
Measurement expressions
Product Version 10.5
Value form
Example
a db value relative to max max-3db ⇒ 3db below maxrng
or min
min+3db ⇒ 3db above minrng
decimal point ( . )
A decimal point ( . ) represents the Y value of the last point
found using a search on the current trace expression of the
goal function. If this is the first search command, then it
represents the Y value of the startpoint of the search.
SLope[(posneg)]
Finds the next maximum slope (positive or negative as
specified) in the specified direction.
[(posneg)] refers to the slope going Positive (P), Negative (N),
or Both (B). If more than the next [#consecutive_points#]
points have zero or opposite slope, the Slope function does
not look any further for the maximum slope.
Positive slope means increasing Y value for increasing indices
of the X expression.
The point found is an artificial point halfway between the two
data points defining the maximum slope.
The default [(posneg)] is Positive.
PEak
Finds the nearest peak. At least [#consecutive_points#] points
on each side of the peak must have Y values less than the
peak Y value.
TRough
Finds nearest negative peak. At least [#consecutive_points#]
points on each side of the trough must have Y values greater
than the trough Y value.
MAx
Finds the greatest Y value for all points in the specified X
range. If more than one maximum exists (same Y values),
then the nearest one is found.
732
PSpice User's Guide
Product Version 10.5
For power users
MAx is not affected by [direction], [#consecutive_points#], or
[repeat:].
MIn
Finds the minimum Y value for all points in the specified X
range.
MIn is not affected by [direction], [#consecutive_points#], or
[repeat:].
POint
Finds the next data point in the given direction.
XValue(value)
Finds the first point on the curve that has the specified X axis
value.
The (value) is a floating-point value or percent of full range.
XValue is not affected by [direction], [#consecutive_points#],
[(range_x [,range_y])], or [repeat:].
(value)
can take any of the following forms:
Value form
Example
a floating number
1e5
100n
1
a percentage of full range 50%
a marked point
x1
y1
PSpice User's Guide
or an expression of
marked points
(x1+x2)/2
a value relative to
startvalue
.-3 ⇒ startvalue -3
a db value relative to
startvalue
.-3db ⇒ 3db below startvalue
.+3 ⇒ startvalue +3
.+3db ⇒ 3db above startvalue
733
Chapter 18
Measurement expressions
Product Version 10.5
Value form
Example
a value relative to max or
min
max-3 ⇒ maxrng -3
min+3 ⇒ minrng +3
Syntax example
The measurement definition is made up of:
■
A measurement name
■
A marked point expression
■
One or more search commands enclosed within curly
braces
This example also includes comments about:
734
■
The measurement definition
■
What arguments it expects when used
■
A sample command line for its usage
PSpice User's Guide
Product Version 10.5
For power users
Any line beginning with an asterisk is considered a comment
line.
Risetime definition
Risetime(1) = x2-x1
*
*#Desc#* Find the difference between the X values
where the trace first
*#Desc#* crosses 10% and then 90% of its maximum
value with a positive
*#Desc#* slope.
*#Desc#* (i.e. Find the risetime of a step
response curve with no
*#Desc#* overshoot. If the signal has overshoot,
use GenRise().)
*
*#Arg1#* Name of trace to search
*
* Usage:
*Risetime(<trace name>)
*
{
1|Search forward level(10%, p) !1
Search forward level(90%, p) !2;
}
The name of the measurement is Risetime. Risetime will take
1 argument, a trace name (as seen from the comments).
The first search function searches forward (positive x
direction) for the point on the trace where the waveform
crosses the 10% point in a positive direction. That point’s X
and Y coordinates will be marked and saved as point 1.
The second search function searches forward in the positive
direction for the point on the trace where the waveform
crosses the 90% mark. That point’s X and Y coordinates will
be marked and saved as point 2.
The marked point expression is x2-x1. This means the
measurement calculates the X value of point 2 minus the X
value of point 1 and returns that number.
PSpice User's Guide
735
Chapter 18
736
Measurement expressions
Product Version 10.5
PSpice User's Guide
Other output options
19
Chapter overview
This chapter describes how to output results in addition to
those normally written to the data file or output file.
PSpice User's Guide
■
Viewing analog results in the PSpice window on
page 738 explains how to monitor the numerical values
for voltages or currents on up to three nets in your circuit
as the simulation proceeds.
■
Writing additional results to the PSpice output file on
page 739 explains how to generate additional line plots
and tables of voltage and current values to the PSpice
output file.
■
Creating test vector files on page 743 explains how to
save digital output states to a file that you can use later as
input to another circuit.
737
Chapter 19
Other output options
Product Version 10.5
Viewing analog results in the PSpice window
Capture provides a special WATCH1 part that lets you monitor
voltage values for up to three nets in your schematic as a DC
sweep, AC sweep or transient analysis proceeds. Results are
displayed in PSpice.
To display voltage values in the PSpice window
1
Place and connect a WATCH1 part (from the PSpice
library SPECIAL.OLB) on an analog net.
2
Double-click the WATCH1 part instance to display the
Parts spreadsheet.
3
In the ANALYSIS property column, type DC, AC, or TRAN
(transient) for the type of analysis results you want to see.
4
Enter values in the LO and HI properties columns to
define the lower and upper bounds, respectively, on the
values you expect to see on this net.
Note: If the results move outside of the specified bounds,
PSpice pauses the simulation so that you can investigate
the behavior.
5
Repeat steps 1 through 4 for up to two more WATCH1
instances.
6
Start the simulation.
For example, in the schematic fragment shown below,
WATCH1 parts are connected to the Mid and Vcc nets. After
738
PSpice User's Guide
Product Version 10.5
Writing additional results to the PSpice output file
starting the simulation, PSpice displays voltages on the Mid
and Vcc nets.
Writing additional results to the PSpice output file
Capture provides special parts that let you save additional
simulation results to the PSpice output file as either
line-printer plots or tables.
To view the PSpice output file after running a simulation:
1
From the Simulation menu, choose Examine Output.
Generating plots of voltage and current values
You can generate voltage and current line-printer plots for any
DC sweep, AC sweep, or transient analysis.
To generate plots of voltage or current to the output file
1
Place and connect any of the following parts (from the
PSpice library SPECIAL.OLB).
Table 19-1
Use this part... To plot this...
VPLOT1
PSpice User's Guide
Voltage on the net that the
part terminal is connected to.
739
Chapter 19
Other output options
Product Version 10.5
Table 19-1
Use this part... To plot this...
VPLOT2
Voltage differential between
the two nets that the part
terminals are connected to.
IPLOT
Current through a net. (Insert
this part in series, like a
current meter.)
2
Double-click the part instance to display the Parts
spreadsheet.
3
Click the property name for the analysis type that you
want plotted: DC, AC, or TRAN.
4
In the columns for the analysis type that you want plotted
(DC, AC or TRAN), type any non-blank value such as Y,
YES or 1.
5
If you selected the AC analysis type, enable an output
format:
a. Click the property name for one of the following
output formats: MAG (magnitude), PHASE, REAL,
IMAG (imaginary), or DB.
b. Type any non-blank value such as Y, YES or 1.
c. Repeat Step a and Step b for as many AC output
formats as you want to see plotted.
Note: If you do not enable a format, PSpice defaults to
MAG.
6
Repeat steps 2 through 5 for any additional analysis
types you want plotted.
Note: If you do not enable an analysis type, PSpice reports
the transient results.
740
PSpice User's Guide
Product Version 10.5
Writing additional results to the PSpice output file
Generating tables of voltage and current values
You can generate tables of voltage and current values on nets
for any DC sweep, AC sweep, or transient analysis.
To generate tables of voltage or current to the output file
1
Place and connect any of the following parts (from the
PSpice library SPECIAL.OLB).
Table 19-2
Use this part... To tabulate this...
VPRINT1
Voltage on the net that the
part terminal is connected to.
VPRINT2
Voltage differential between
the two nets that the part
terminals are connected to.
IPRINT
Current through a cut in the
net. (Insert this part in series,
like a current meter.)
2
Double-click the part instance to display the Parts
spreadsheet.
3
Click the property name for the analysis type that you
want tabulated: DC, AC, or TRAN.
4
In the columns for the analysis type that you want plotted
(DC, AC or TRAN), type any non-blank value such as Y,
YES or 1.
5
If you selected the AC analysis type, enable an output
format.
a. Click the property name for one of the following
output formats: MAG (magnitude), PHASE, REAL,
IMAG (imaginary), or DB.
b. Type any non-blank value such as Y, YES or 1.
PSpice User's Guide
741
Chapter 19
Other output options
Product Version 10.5
c. Repeat Step a and Step b for as many AC output
formats as you want to see tabulated.
Note: If you do not enable a format, PSpice defaults to
MAG.
6
Repeat steps 2 through 5 for any additional analysis
types you want plotted.
Note: If you do not enable an analysis type, PSpice reports
the transient results.
Generating tables of digital state changes
You can generate a table of digital state changes during a
transient analysis for any net.
To generate a table of digital state changes to the output
file
1
742
Place a PRINTDGTLCHG part
(from the PSpice
library SPECIAL.OLB) and connect it to the net that you
are interested in.
PSpice User's Guide
Product Version 10.5
Writing additional results to the PSpice output file
Creating test vector files
Capture provides a special VECTOR part that lets you save
digital simulation results to a vector file. Whenever any net
with an attached VECTOR part changes state, PSpice writes
a line of time-value data to the vector file using the same
format as the file stimulus device. This means that you can
use the vector file to drive inputs for another simulation. To find
out about vector file syntax, refer to the online PSpice
Reference Guide.
To find out about setting up digital stimuli, see Defining a
digital stimulus on page 543.
To generate a test vector file from your circuit
1
Place a VECTORn part (from the PSpice library
SPECIAL.OLB) and connect it to a wire or bus at the
output of a digital part instance.
2
Double-click the VECTORn part instance to display the
Parts spreadsheet.
double-click here to
edit the POS property
double-click here to
edit all properties
3
Set the part properties as described below.
Table 19-3
PSpice User's Guide
For this
property...
Define this...
POS
Column position in the file.
Valid values range from 1 to
255.
743
Chapter 19
Other output options
Product Version 10.5
Table 19-3
For this
property...
Define this...
FILE
Name of the vector file. If left
blank, PSpice A/D creates a
file named
SCHEMATIC_NAME.VEC.
RADIX
If the VECTOR part is
attached to a bus, the
numerical notation for a bus.
Valid values are B[inary],
O[ctal], and H[ex].
BIT
If the VECTOR part is
attached to a wire, the bit
position within a single hex or
octal digit.
SIGNAMES
Names of the signals that
appear in the header of the
file. If left blank, PSpice
defaults to the following:
■
For a wire, the label
(name) on the wire.
■
For a bus, a name derived
from the position of each
signal in the bus (from
MSB to LSB).
Note: You can group separate signal values to form a hex
or octal value by specifying the same POS property and
defining RADIX as Hex or Octal. Define the bit position
within the value using the BIT property.
4
744
Repeat steps 1 through 3 for as many test vectors as you
want to create.
PSpice User's Guide
Setting initial state
A
Appendix overview
This appendix includes the following sections:
PSpice User's Guide
■
Save and load bias point on page 746
■
Setpoints on page 748
■
Setting initial conditions on page 750
745
Chapter A
Setting initial state
Product Version 10.5
Save and load bias point
Save Bias Point and Load Bias Point are used to save and
restore bias point calculations in successive PSpice
simulations.
Note: Save/Load Bias Point feature is not available in
PSpice A/D Basics.
Saving and restoring bias point calculations can decrease
simulation times when large circuits are run multiple times and
can aid convergence. If the circuit uses high gain components,
or if the circuit’s behavior is nonlinear around the bias point,
this feature is not useful.
Save/Load Bias Point affect the following types of analyses:
■
transient
■
DC
■
AC
Save bias point
Save bias point is a simulation control function that allows you
to save the bias point data from one simulation for use as initial
conditions in subsequent simulations. Once bias point data is
saved to a file, you can use the load bias point function to use
the data for another simulation.
To use save bias point
1
In the Simulation Settings dialog box, click the Analysis
tab.
See Setting up analyses on page 373 for a description of
the Analysis Setup dialog box.
746
2
Under Options, select Save Bias Point.
3
Complete the Save Bias Point dialog box.
4
Click OK.
PSpice User's Guide
Product Version 10.5
Appendix overview
Load bias point
Load bias point is a simulation control function that allows you
to set the bias point as an initial condition. A common reason
for giving PSpice initial conditions is to select one out of two or
more stable operating points (set or reset for a flip-flop, for
example).
To use load bias point
1
Run a simulation using the Save Bias Point option in the
Simulation Settings dialog box.
See Setting up analyses on page 373 for a description of
the Analysis Setup dialog box.
PSpice User's Guide
2
Before running another simulation, click the Analysis tab
in the Simulation Settings dialog box.
3
Under Options, select Load Bias Point.
4
Specify a bias point file to load. Include the path if the file
is not located in your working directory, or use the Browse
button to find the file.
5
Click OK.
747
Chapter A
Setting initial state
Product Version 10.5
Setpoints
Pseudocomponents that specify initial conditions are called
setpoints. These apply to the analog portion of your circuit.
Figure A-1 Setpoints.
The example in Figure A-1 includes the following:
IC1
IC2
a one-pin symbol that allows you to
set the initial condition on a net for
both small-signal and transient bias
points
a two-pin symbol that allows you to
set initial condition between two nets
Using IC symbols sets the initial conditions for the bias point
only. It does not affect the DC sweep. If your circuit design
contains both an IC symbol and a NODESET symbol for the
same net, the NODESET symbol is ignored.
To specify the initial condition, edit the value of the VALUE
property to the desired initial condition. PSpice attaches a
voltage source with a 0.0002 ohm series resistance to each
net to which an IC symbol is connected. The voltages are
clamped this way for the entire bias point calculation.
NODESET1 is a one-pin symbol which helps calculate the
bias point by providing a initial guess for some net.
NODESET2 is a two-pin symbol which helps calculate the
bias point between two nets. Some or all of the circuit’s nets
may be given an initial guess. NODESET symbols are
effective for the bias point (both small-signal and transient bias
points) and for the first step of the DC sweep. It has no effect
during the rest of the DC sweep or during the transient
analysis itself.
748
PSpice User's Guide
Product Version 10.5
Appendix overview
Unlike the IC pseudocomponents, NODESET provides only
an initial guess for some net voltages. It does not clamp those
nodes to the specified voltages. However, by providing an
initial guess, NODESET symbols may be used to break the tie
(in a flip-flop, for instance) and make it come up in a desired
state. To guess at the bias point, enter the initial guess in the
Value text box for the VALUE property. PSpice A/D attaches a
voltage source with a 0.0002 ohm series resistance to each
net to which an IC symbol is connected.
These pseudocomponents are netlisted as PSpice A/D .IC
and .NODESET commands. Refer to these commands in the
online PSpice Reference Guide for more information.
Setpoints can be created for inductor currents and capacitor
voltages using the IC property described in Setting initial
conditions on page 750.
PSpice User's Guide
749
Chapter A
Setting initial state
Product Version 10.5
Setting initial conditions
The IC property allows initial conditions to be set on
capacitors and inductors. These conditions are applied during
all bias point calculations. However, if you select the Skip
Initial Transient Solution check box in the Transient Analysis
Setup dialog box, the bias point calculation is skipped and the
simulation proceeds directly with transient analysis at
TIME=0. Devices with the IC property defined start with the
specified voltage or current value; however, all other such
devices have an initial voltage or current of 0.
Note: Skipping the bias point calculation can make the
transient analysis subject to convergence problems.
Applying an IC property for a capacitor has the same effect as
applying one of the pseudocomponents IC1 or IC2 across its
nodes. PSpice attaches a voltage source with a 0.002 ohm
series resistance in parallel with the capacitor. The IC property
allows the user to associate the initial condition with a device,
while the IC1 and IC2 pseudocomponents allow the
association to be with a node or node pair. See Setpoints on
page 748 for more information about IC1 and IC2.
In the case of initial currents through inductors, the
association is only with a device, and so there are no
corresponding pseudocomponents. The internal
implementation is analogous to the capacitor. PSpice
attaches a current source with a 1 Gohm parallel resistance in
series with the inductor.
750
PSpice User's Guide
Convergence and “time step too
small errors”
B
Appendix overview
This appendix discusses common errors and convergence
problems in PSpice.
PSpice User's Guide
■
Introduction on page 752
■
Diagnostics on page 756
■
Bias Point (DC) Convergence on page 757
■
DC Sweep Convergence on page 762
■
Transient Convergence on page 763
751
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
Introduction
In order to calculate the bias point, DC sweep and transient
analysis for analog devices PSpice must solve a set of
nonlinear equations which describe the circuit's behavior. This
is accomplished by using an iterative technique—the
Newton-Raphson algorithm—which starts by having an initial
approximation to the solution and iteratively improves it until
successive voltages and currents converge to the same result.
In a few cases PSpice cannot find a solution to the nonlinear
circuit equations. This is generally called a “convergence
problem” because the symptom is that the Newton-Raphson
repeating series cannot converge onto a consistent set of
voltages and currents. The following discussion gives some
background on the algorithms in PSpice and some guidelines
for avoiding convergence problems.
The transient analysis has the additional possibility of being
unable to continue because the time step required becomes
too small from something in the circuit moving too fast. This is
also discussed below.
Note: The AC and noise analyses are linear and do not use
an iterative algorithm, so the following discussion does
not apply to them. Digital devices are evaluated using
boolean algebra; this discussion does not apply to
them either.
Newton-Raphson requirements
The Newton-Raphson algorithm is guaranteed to converge
to a solution. However, this guarantee has some conditions:
1
The nonlinear equations must have a solution.
2
The equations must be continuous.
3
The algorithm needs the equations' derivatives.
4
The initial approximation must be close enough to the
solution.
Each of these can be taken in order. Remember that the
PSpice algorithms are used in computer hardware that has
752
PSpice User's Guide
Product Version 10.5
Appendix overview
finite precision and finite dynamic range that produce these
limits:
■
Voltages and currents in PSpice are limited to +/-1e10
volts and amps.
■
Derivatives in PSpice are limited to 1e14.
■
The arithmetic used in PSpice is double precision and
has 15 digits of accuracy.
Is there a solution?
Yes, for any physically realistic circuit. However, it is not
difficult to set up a circuit that has no solution within the limits
of PSpice numerics.
Consider, for example, a voltage source of one megavolt
connected to a resistor of one micro-ohm. This circuit does not
have a solution within the dynamic range of currents (+/- 1e10
amps). Here is another example:
V1
1,
D1
1,
.MODEL
0
5v
0
DMOD
DMOD(IS=1e-16)
The problem here is that the diode model has no series
resistance. To find out more about the diode equations, refer
to the Analog Devices chapter in the online PSpice
Reference Guide.
It can be shown that the current through a diode is:
I = IS*eV/(N*k*T/q)
N defaults to one and k*T at room temperature is about .025
volts. So, in this example the current through the diode would
be:
I = 1e-16*e200 = 7.22e70 amps
This circuit also does not have a solution within the limits of the
dynamic range of PSpice. In general, be careful of
components without limits built into them. Extra care is
needed when using the expressions for controlled sources
(such as for behavioral modeling). It is easy to write
expressions with very large values.
PSpice User's Guide
753
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
Are the equations continuous?
The device equations built into PSpice are continuous. The
functions available for behavioral modeling are also
continuous (there are several functions, such as int(x), which
cannot be added because of this). So, for physically realistic
circuits the equations can also be continuous. Exceptions that
come are usually from exceeding the limits of the numerics in
PSpice. This example tries to approximate an ideal switch
using the diode model:
.MODEL DMOD(IS=1e-16 N=1e-6)
The current through this diode is:
I = 1e-16*eV/(N*.025) = 1e-16*eV/25e-9
Because the denominator in the exponential is so small, the
current I is essentially zero for V < 0 and almost infinite for
V > 0. Even if there are external components that limit the
current, the “knee” of the diode's I-V curve is so sharp that it
is almost a discontinuity.
Note: Avoid unrealistic model parameters. Behavioral
modeling expressions need extra care.
Are the derivatives correct?
The device equations built into PSpice include the derivatives,
and these are correct. Depending on the device, the physical
meaning of the derivatives can be small-signal conductance,
transconductance or gain.
Unrealistic model parameters can exceed the limit of 1e14,
but it requires some effort. The main thing to look at is the
behavioral modeling expressions, especially those having
denominators.
Discontinuities in models characteristics and their derivatives
cause:
754
1
Ambiguity in calculation of derivatives at point of
discontinuity.
2
Conductance calculated in nth iteration cannot become a
good guess for next iteration.
PSpice User's Guide
Product Version 10.5
Appendix overview
3
Sudden switching of operating regions (example diode
switching from off to on) and hence false convergence.
Note: Transient analysis convergence failures are usually due
to model discontinuities or unrealistic circuit, source, or
parasitic modeling.
Is the initial approximation close enough?
Newton-Raphson is guaranteed to converge only if the
analysis is started close to the answer. Also, there is no
measurement that can tell how close is close enough.
PSpice gets around this by making heavy use of continuity.
Each analysis starts from a known solution and uses a
variable step size to find the next solution. If the next solution
does not converge PSpice reduces the step size, falls back
and tries again.
Incorrect initial estimates can cause convergence failure or
even false convergence. Consider following scenarios:
PSpice User's Guide
■
Power electronic circuits may NOT require tight
current/voltage tolerances. Setting the value of ABSTOL
to 1u will help in the case of circuits that have currents
that are larger than several amps.
■
Unless the circuit conducts kilo-Amperes of current,
however, setting ABSTOL to a value that is greater than
1u will cause more convergence problems than it will
solve.
■
PSpice does not always converge when relaxed
tolerances are used. For example, setting the tolerance
option, RELTOL, to a value which is greater than .01 can
actually cause convergence problems
■
Setting GMIN to a value between 1n and 10n will often
solve convergence problems.
■
Setting GMIN to a value, which is greater than 10n, may
cause convergence problems.
755
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
Diagnostics
If PSpice encounters a convergence problem it inserts into the
output file a message that looks like the following.
ERROR -- Convergence problem in transient analysis at Time = 7.920E-03
Time step = 47.69E-15, minimum allowable step size = 300.0E-15
These voltages failed to converge:
V(x2.23) =
1230.23 / -68.4137
V(x2.25) =
-1211.94 / 86.6888
These supply currents failed to converge:
I(X2.L1)
=
-36.6259 / 2.25682
I(X2.L2)
=
-36.5838 / 2.29898
These devices failed to converge:
X2.DCR3
X2.DCR4
x2.ktr
X2.Q1
X2.Q2
Last node voltages tried were:
NODE
VOLTAGE
NODE
VOLTAGE NODE
VOLTAGE
NODE
VOLTAGE
(
1) 25.2000
(
3)
4.0000
(
4) 0.0000
(
6)
25.2030
(x2.23) 1230.2000 (X2.24)
9.1441
(x2.25) -1211.9000 (X2.26)
256.9700
(X2.28) -206.6100 (X2.29)
75.4870 (X2.30) -25.0780
(X2.31)
26.2810
(X3.34) 1.771E-06 (X3.35)
1.0881
(X3.36) .4279
(X2.XU1.6) 1.2636
The message always includes the banner (ERROR -convergence problem ...) and the trailer (Last node
voltages tried were ...). It cannot include all three of
the middle blocks.
The Last node voltages tried... trailer shows the
voltages tried at the last Newton-Raphson iteration. If any of
the nodes have unreasonable large values this is a clue that
these nodes are related to the problem. “These voltages failed
to converge” lists the specific nodes which did not settle onto
consistent values. It also shows their values for the last two
iterations. “These supply currents failed converge” does the
same for currents through voltage sources and inductors. If
any of the listed numbers are +/- 1e10 then that is an
indication that the value is being clipped from an
unreasonable value. Finally, “These devices failed to
converge” shows devices whose terminal currents or core
fluxes did not settle onto consistent values.
The message gives a clue as to the part of the circuit which is
causing the problem. Looking at those devices and/or nodes
for the problems discussed above is recommended.
756
PSpice User's Guide
Product Version 10.5
Bias Point (DC) Convergence
Bias Point (DC) Convergence
The hardest part of the whole process is getting started, that
is, finding the bias point. PSpice first tries with the power
supplies set to 100%. A solution is not guaranteed, but most
of the time the PSpice algorithm finds one. If not, then the
power supplies are cut back to almost zero. They are cut to a
level small enough that all nonlinearities are turned off.
When the circuit is linear a solution can be found (very near
zero, of course). Then, PSpice works its way back up to 100%
power supplies using a variable step size.
Once a bias point is found, the transient analysis can be run.
It starts from a known solution (the bias point) and steps
forward in time. The step size is variable and is reduced as
needed to find further solutions.
In case the circuit fails to converge, you should first check the
circuit topology and connectivity, followed by modelling of
circuit components, and finally check if Pspice options are set
properly.
Checking circuit topology and connectivity
■
Make sure that all of the circuit connections are valid.
Check for incorrect node numbering or dangling nodes.
Also, verify component polarity.
■
Check for syntax mistakes. Make sure that you used the
correct PSPICE units (i.e. MEG for 1E6, not M, which
means mili in simulations).
■
PSpice checks for the following conditions and provides
messages if they occur:
❑
PSpice User's Guide
“Floating node" or "No DC path to ground"
messages:
❍
Make sure that there's a DC path from every
node to ground.
❍
Make sure that there are at least two
connections at every node.
757
Chapter B
Convergence and “time step too small errors”
❑
Product Version 10.5
❍
Make sure that capacitors and/or current
sources are not connected in series.
❍
Make sure that no (groups of) nodes are isolated
from ground by current sources and/or
capacitors.
"Voltage source or inductor loop" message:
❍
Make sure that there are no loops of only
inductors and/or voltage sources.
■
Place the ground (node 0) somewhere in the circuit. Be
careful when you use floating grounds (e.g. chassis
ground); you may need to connect a large resistor from
the floating node to ground. All nodes will be reported as
floating if "0 ground" is not used.
■
Make sure that voltage/current generators use realistic
values, and verify that the syntax is correct.
■
Make sure that dependent source gains are correct, and
that E/G element expressions are reasonable. Verify that
division by zero or LOG(0) cannot occur.
■
Make sure that there are no unrealistic model
parameters; especially if you have manually entered the
model into the netlist.
■
Avoid using digital components, unless really necessary.
Initialize the nodes with valid digital value to ensure the
state is not ambiguous.
Modelling circuit components
■
Semiconductors
The first consideration for semiconductors is to avoid
physically unrealistic model parameters. As PSpice steps
the power supplies up, it has to step carefully through the
turn on transition for each device. In the diode example
above, for the setting N=1e-6, the knee of the I-V curve
would be too sharp for PSpice to maintain its continuity
within the power supply step size limit of 1e-6.
■
758
Behavioral modeling expressions
PSpice User's Guide
Product Version 10.5
Bias Point (DC) Convergence
Range limits: Voltages and currents in PSpice are
limited to the range +/- 1e10. Care must be taken that the
output of expressions falls within this range. This is
especially important when one is building an electrical
analog of a mechanical, hydraulic or other type of system.
Source limits: Another consideration is that the
controlled sources must turn off when the supplies are
almost 0 (.001%). There is special code in PSpice which
"squelches" the controlled sources in a continuous way
near 0 supplies. However, care should still be taken using
expressions that have denominators. Take, for example, a
constant power load:
GLOAD 3, 5 VALUE = {2Watts/V(3,5)}
The first repeating series starts with V(3,5) = 0 and the
current through GLOAD would be infinite (actually, the
code in PSpice which does the division clips the result to
a finite value). The "squelching" code is required to be a
smooth and well-behaved function.
Note: The "squelching" code cannot be "strong" enough
to suppress dividing by 0.
The result is that GLOAD does not turn off near 0 power
supplies. A better way is described in the application note
Modeling Constant Power Loads. The "squelching" code
is sufficient for turning off all expressions except those
having denominators. In general, though, it is good
practice to constrain expressions having the LIMIT
function to keep results within physically realistic bounds.
Example: A first approximation to an OPAMP that has an
open loop gain of 100,000 is:
VOPAMP 3, 5 VALUE = {V(in+,in-)*1e5}
This has the undesirable property that there is no limit on
the output.
A better expression is:
VOPAMP 3, 5 VALUE = +
{LIMIT(V(in+,in-)*1e5,15v,-15v}
where the output is limited to +/- 15 volts.
■
PSpice User's Guide
Unguarded p-n junctions
759
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
A second consideration is to avoid "unguarded" p-n
junctions (no series resistance).
■
No leakage resistance
A third consideration is to avoid situations, which could
have an ideal current source pushing current into a
reverse-biased p-n junction without a shunt resistance.
p-n junctions in PSpice have (almost) no leakage
resistance and would cause the junction's voltage to go
beyond 1e10 volts.
■
Switches
PSpice switches have gain in their transition region. If
several are cascaded then the cumulative gain can easily
exceed the derivative limit of 1e14. This can happen
when modeling simple logic gates using totem-pole
switches and there are several gates cascaded in series.
Usually a cascade of two switches works but three or
more can cause trouble.
PSpice Options
■
Increase ITL1 to 400 in the .OPTIONS statement.
Example: .OPTIONS ITL1=400
This increases the number of DC iterations that PSpice
will perform before it gives up. In all but the most complex
circuits, further increases in ITL1 won't typically aid
convergence.
■
Add .NODESETs
Example: .NODESET V(6)=0
Use NODESETs to set node voltages to the nearest
reasonable guess at their DC values, particularly at
nodes that are isolated by high impedances, and at nodes
that are inputs to high gain devices. NODESETs do not
"fix" the voltages at these nodes. They hold these
voltages at the specified value while the rest of the circuit
converges to a reasonably stable point, and then
"releases" these voltages for a few more iterations to find
the final, complete solution. Removing these voltages
760
PSpice User's Guide
Product Version 10.5
Bias Point (DC) Convergence
from the initial iterations, when voltages and currents are
varying widely helps PSpice achieve convergence.
■
STEPGMIN
Specifying the circuit analysis option STEPGMIN enables
this (either using .OPTION STEPGMIN in the netlist, or by
making the appropriate choice from the PSpice/Edit
Simulation Profile… menu command, Options tab). When
enabled, the GMIN stepping algorithm is applied after the
circuit fails to converge with the power supplies at 100
percent, and if GMIN stepping also fails, the supplies are
then cut back to almost zero and then stepped up.
GMIN stepping attempts to find a solution by starting the
repeating cycle with a large value of GMIN, initially
1.0e10 times the nominal value. If a solution is found at
this setting it then reduces GMIN by a factor of 10, and
tries again. This continues until either GMIN is back to the
nominal value, or until PSpice fails to converge at one of
the GMIN values on the way. In the latter case, GMIN is
restored to the nominal value and the power supplies are
stepped.
■
Power supply stepping
As previously discussed, PSpice uses a proprietary
algorithm which finds a continuous path from zero power
supplies levels to 100%. It starts at almost zero (.001%)
power supplies levels and works its way back up to the
100% levels. The minimum step size is 1e-6 (.0001%).
The first repeating series of the first step starts at zero for
all voltages. So modeling expressions, especially those
having denominators that include voltages should be
checked carefully.
■
Set PREORDER in Simulation Profiles options
This is important while editing schematic for marginally
convergent circuits. Setting PREORDER reduces
dependency on the netlisting order thereby ensuring that
the non convergence error does not occur because of the
change in the netlisting order.
PSpice User's Guide
761
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
DC Sweep Convergence
The DC sweep uses a hybrid approach. It uses the bias point
algorithm (varying the power supplies) to get started. For
subsequent steps it uses the previous solution as the initial
approximation. The sweep step is not variable, however. If a
solution cannot be found at a step then the bias point
algorithm is used for that step.
The whole process relies heavily on continuity. It also requires
that the circuit be linear when the supplies are turned off.
Circuit topology and connectivity
This is same as in DC analysis. See Checking circuit topology
and connectivity on page 757.
Modelling Checks
This is same as in DC analysis. Modelling circuit components
on page 758.
PSpice Options
■
Set ITL2=100 in the .OPTIONS statement.
Example: .OPTIONS ITL2=100
This increases the number of DC iterations that PSpice
will attempt before it gives up.
■
Increase or decrease the step values, which are used in
the .DC sweep.
Example:
.DC VCC 0 1 .1 becomes .DC VCC 0 1 .01
Discontinuities in the PSpice models can cause
convergence problems. The use of larger steps may help
to bypass the discontinuities, while the use of smaller
steps may help PSpice find the intermediate answers,
which will be used to find the point, which doesn't
converge. In some cases, smaller steps can improve
762
PSpice User's Guide
Product Version 10.5
Transient Convergence
convergence, because they help PSpice find a "path"
from the valid DC solution at one point to the valid solution
at the next.
■
Do not use the DC sweep analysis.
Example:
.DC VCC 0 5 .1
VCC 1 0
becomes
.TRAN .01 1
VCC 1 0 PULSE 0 5 0 1
In many cases, it is preferable to use the transient
analysis to ramp the appropriate voltage and/or current
sources. The transient analysis tends to be more robust,
and is sometimes faster.
Transient Convergence
The transient analysis starts using a known solution - the bias
point. It then uses the most recent solution as the first guess
for each new time point. If necessary, the time step is cut back
to keep the new time point close enough that the first guess
allows the Newton-Raphson repeating series to converge.
The time step is also adjusted to keep the integration of
charges and fluxes accurate enough.
In theory the same considerations which were noted for the
bias point calculation apply to the transient analysis. However,
in practice they show up during the bias point calculation first
and, hence, are corrected before a transient analysis is run.
The transient analysis can fail to complete if the time step gets
too small. This can have two different effects:
1
The Newton-Raphson iterations would not converge even
for the smallest time step size, or
2
Something in the circuit is moving faster than can be
accommodated by the minimum step size.
The message PSpice puts into the output file specifies which
condition occurred.
PSpice User's Guide
763
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
Circuit topology and connectivity
■
Avoid using digital components, unless really necessary.
Initialize the nodes with valid digital value to ensure no
ambiguous state. These can cause time-step issues
(time-step may unnecessary go too small) and hence
transient convergence issue.
■
Use RC snubbers around diodes.
■
Add Capacitance for all semiconductor junctions (if no
specific value is known: CJO=3pF for diodes, CJC &
CJE=5pF for BJTs, CGS and CGD=5pF for JFETs and
GaAsFETs, CGDO & CGSO=5pF for MOSFETs if no
specific value is known).
■
Add realistic circuit and element parasitics.
■
Look for waveforms that transition vertically (up or down)
at the point during which the analysis halts. These are the
key nodes, which should be examined for problems.
■
Increase the rise/fall times of the PULSE sources; e.g.
from 1f to 1u.
Example:
VCC 1 0 PULSE 0 1 0 1f 1f
becomes
VCC 1 0 PULSE 0 1 0 1U 1U
An effort should be made to smooth strong
non-linearities. The pulse times should be realistic, not
ideal. If no rise or fall time values are given, or if 0 is
specified, the rise and fall times will be set to the TSTEP
value in the .TRAN statement (set in the Output File
Options of the Time Domain (Transient) analysis settings
in the simulation profile.
■
Ensure that there is no unreasonably large capacitor or
inductor
If the transient analysis fails at the first time point then
usually there is an unreasonably large capacitor or
inductor. Usually this is due to a typographical error.
Consider the following capacitor:
C 1 3, 0 1Ouf
764
PSpice User's Guide
Product Version 10.5
Transient Convergence
"1O" (has the letter O) should have been "10." This capacitor
has a value of one farad, not 10 microfarads. An easy way to
catch these is to use the LIST option (on the .OPTIONS
command).
LIST
The LIST option can echo back all the devices into the output
file that have their values in scientific notation.
That makes it easy to spot any unusual values. This kind of
problem does not show up during the bias point calculation
because capacitors and inductors do not participate in the
bias point.
Similar comments apply to the parasitic capacitance
parameters in transistor (and diode) models. These are
normally echoed to the output file (the NOMOD option
suppresses the echo but the default is to echo). As in the LIST
output, the model parameters are echoed in scientific notation
making it easy to spot unusual values. A further diagnostic is
to ask for the detailed operating bias point (.TRAN/OP)
information.
.TRAN/OP
This lists the small-signal parameters for each semiconductor
device including the calculated parasitic capacitances.
Realistically Model Circuit; add parasitics, especially stray/junction capacitance
The idea here is to smooth any strong non-linearties or
discontinuities. This may be accomplished via the addition of
capacitance to various nodes and verifying that all
semiconductor junctions have capacitance. Other tips include:
■
Bipolar transistors substrate junction
The UC Berkeley SPICE contains an unfortunate
convention for the substrate node of bipolar transistors.
The collector-substrate p-n junction has no DC
component. If the capacitance model parameters are
PSpice User's Guide
765
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
specified (e.g., CJS) then the junction has
(voltage-dependent) capacitance but no DC current. This
can lead to a sneaky problem: if the junction is
inadvertently forward-biased it can create a very large
capacitance. The capacitance goes as a power of the
junction voltage. Normal junctions cannot sustain much
forward voltage because a large current flows. The
collector-substrate junction is an exception because it
has no DC current. If this happens it usually shows up at
the first time step. It can be spotted turning on the detailed
operating point information (.TRAN/OP) and looking at
the calculated value of CJS for bipolar transistors. The
whole problem can be prevented by using the PSpice
model parameter ISS. This parameter "turns on" the DC
current for the substrate junction.
■
Parasitic capacitances
It is important that switching times be nonzero. This is
assured if devices have parasitic capacitances. The
semiconductor model libraries in PSpice have such
capacitances. If switches and/or controlled sources are
used, then care should be taken to assure that no
sections of circuitry can try to switch in zero time. In
practice this means that if any positive feedback loops
exist (such as a Schmidt trigger built out of switches) then
such loops should include capacitances.
Another way of saying all this is that during transient
analysis the circuit equations must be continuous over
time (just as during the bias point calculation the
equations must be continuous with the power supply
level).
■
Inductors and transformers
While the impedance of capacitors gets lower at high
frequencies (and small time steps) the impedance of
inductors gets higher.
Note: The inductors in PSpice have an infinite
bandwidth.
Real inductors have a finite bandwidth due to eddy
current losses and/or skin effect. At high frequencies the
effective inductance drops.
766
PSpice User's Guide
Product Version 10.5
Transient Convergence
Another way to say this is that physical inductors have a
frequency at which their Q begins to roll off. The inductors
in PSpice have no such limit. This can lead to very fast
spikes as transistors (and diodes) connected to inductors
turn on and off. The fast spikes, in turn, can force PSpice
to take unrealistically small time steps.
■
It is recommended that all inductors have a parallel
resistor (series resistance is good for modeling DC
effects but does not limit the inductor's bandwidth). The
parallel resistor gives a good model for eddy current loss
and limits the bandwidth of the inductor. The size of
resistor should be set to be equal to the inductor's
impedance at the frequency at which its Q begins to roll
off. The value of this resistor can be calculated using the
following formula:
R = 2×Π×f×L
where f is the roll-off frequency.
Adding parallel resistors limits the inductor impedance at
high frequencies.
Example:
A common one milli-henry iron core inductor begins to roll
off at no less than 100KHz. A good resistor value to use
in parallel is then R = 2*p*100e3*.001 = 628 ohms. Below
the roll-off frequency the inductor dominates; above it the
resistor does. This keeps the width of spikes from
becoming unreasonably narrow.
PSpice options
TIME, the simulation time during transient analysis, is a
double precision variable which gives it about 15 digits of
accuracy. The dynamic range is set to be 15 digits minus the
number of digits of accuracy required by RELTOL. For a
default value of RELTOL = .001 (.1% or 3 digits) this gives 15-3
= 12 digits. This means that the minimum time step is the
overall run time (TSTOP) divided by 1e12. The dynamic range
is large but finite.
It is possible to exceed this dynamic range in some circuits.
Consider, for example, a timer circuit which charges up a
PSpice User's Guide
767
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
100uF capacitor to provide a delay of 100 seconds. At a
certain threshold a comparator turns on a power MOSFET.
The overall simulation time is 100 seconds. For default
RELTOL this gives us a minimum time step of 100
picoseconds. If the comparator and other circuitry has
portions that switch in a nanosecond then PSpice needs steps
of less than 100 picoseconds to calculate the transition
accurately.
■
Set RELTOL=.01 in the .OPTIONS statement.
Example:
.OPTIONS RELTOL=.01
This option is encouraged for most simulations, since the
reduction of Reltol can increase the simulation speed by
10 to 50%. Only a minor loss in accuracy usually results.
A useful recommendation is to set Reltol to .01 for initial
simulations, and then reset it to its default value of .001
when you have the simulation running the way you like it
and a more accurate answer is required. Setting Reltol to
a value less than .001 is generally not required.
■
Reduce the accuracy of ABSTOL/VNTOL if
current/voltage levels allow it.
Example:
.OPTION ABSTOL=1N VNTOL=1M
Abstol and Vntol should be set to about 8 orders of
magnitude below the level of the maximum voltage and
current. The default values are Abstol=1pA and
Vntol=1uV. These values are generally associated with IC
designs.
■
Increase ITL4, but to no more than 100, in the .OPTIONS
statement.
Example:
.OPTIONS ITL4=40
This increases the number of transient iterations that
PSpice will attempt at each time point before it gives up.
This is particularly effective at solving convergence
problems when the simulation needs to cover a long time
period, and fast transitions occur within the circuit during
768
PSpice User's Guide
Product Version 10.5
Transient Convergence
that time. Values greater than 100 won't usually bring
convergence; unnecessarily large values can cause.
■
Skipping the bias point
The SKIPBP option for the transient analysis skips the
bias point calculation. In this case the transient analysis
has no known solution to start from and, therefore, is not
assured of converging at the first time point. Because of
this, its use is not recommended. Its inclusion in PSpice
is to maintain compatibility with UC Berkeley SPICE.
SKIPBP has the same meaning as UIC in Berkeley
SPICE. UIC is not needed in order to specify initial
conditions.
It should be used as a last resort if there is trouble getting
the transient analysis to start because the DC operating
point can't be calculated. The initial guess for dc could be
made from results of such transient analysis; and then
transient analysis could be re-run with operating point.
You should add any applicable .IC and IC= initial
conditions statements to assist in the initial stages of the
transient analysis. Be careful when you set initial
conditions, for a poor setting may cause convergence
difficulties.
■
Increasing the ABSTOL and CHGTOL
While modeling a mechanical system with an RC circuit,
where capacitors are in the order of Farad and current
impulses is around 10x A, increase CHGTOL and
ABSTOL by six order of magnitude. For example, change
CHGTOL from 0.01e-012 to0.01e-006. Simulate the
circuit and then start tightening the ABSTOL and
CHGTOL values until a convergence error is generated.
Once a convergence error is generated, you can revert
one step to get the solution.
■
Set the DIGSTEPBACK option
.OPTIONS DIGSTEPBACK
Setting this option might prove useful in cases where your
have convergence problems in a circuits with digital
components and you are trying to converge using
Solver 1.
PSpice User's Guide
769
Chapter B
Convergence and “time step too small errors”
Product Version 10.5
Though setting DIGSTEPBACK option might work, it is
recommended that you should use solver 0 simulation
algorithm to obtain a solution.
Tip
Solver 1 and Solver 0 are two matrix solving
algorithms used by PSpice. By default, Solver 1 that
has better convergence property, is used. But at
times, for a circuit with convergence problems
changing the simulation algorithm to Solver 0 helps.
To change the simulation algorithm from Solver 1 to
Solver 0, open the circuit in the schematic editor.
From the PSpice menu choose Edit Simulation
Profile. In the Simulation Settings dialog box,
select the Options tab. Select the Advanced
Options button. In the Advanced Analog Options
dialog box, change the Simulation algorithm from
default to 0.
770
PSpice User's Guide
Importing Spice Models
C
Appendix Overview
This appendix covers the process to be followed for importing
Spice models downloaded from a web site, into PSpice and
making them ready to be used in a circuit. The sections
covered in this appendix are:
PSpice User's Guide
■
Introduction on page 772
■
Importing text models on page 772
■
Generating Part Symbols on page 773
■
Configuring new model library on page 779
■
Editing Model Editor created symbols on page 781
771
Chapter C
Importing Spice Models
Product Version 10.5
Introduction
Usually, the Spice models downloaded from a Vendor’s web
site cannot be used directly in PSpice. This document covers
the steps to be covered before you can successfully use the
downloaded models for designing your circuits.
Before you can use the simulation models downloaded from a
web site in your design, you need to perform following steps:
■
Importing text models
■
Generating Part Symbols
■
Configuring new model library
Importing text models
To import the downloaded Spice models into PSpice, you
need to perform the following steps.
1
Rename the downloaded model to have the .MOD
extension.
Note: Renaming is required only if the downloaded
model does not have a .MOD extension. For example,
renaming will be required if the download model has a .txt
extension.
2
Launch the Model Editor.
3
Open a new or your custom model library.
4
From the Model menu, choose Import.
5
In the Open dialog box, select the downloaded model with
the .MOD extension and select Open.
Note: Only the first model in the .MOD file is imported.
Therefore, it is recommended that the .MOD file should
not have more than one model.
6
772
From the file Menu, choose Save As. In the Save As
dialog box, specify the name and location of new model
library as
PSpice User's Guide
Product Version 10.5
Generating Part Symbols
<installation_directory>\tools\Pspice\l
ibrary\userlib.
Note: It is preferable to create you own USERLIB library
folder to store all of your custom part and model libraries
for better library management. It is important that you
back up your custom libraries and projects on a regular
basis to avoid loss of work.
Generating Part Symbols
After you have imported the downloaded model into PSpice,
you need to generate part symbols for the model. You can
associate a model to a symbol either by Creating New
Symbols or by Using symbols from an existing symbol library
or by Using Model Import wizard.
Creating New Symbols
You can create Capture symbols for the imported/downloaded
models. Using Model Editor you can either create parts for all
the models in a library or you can enable the auto part
generation feature in Model Editor, such that part is created
every time you save a model.
Creating symbol for the complete library
PSpice User's Guide
1
Open the Model Editor.
2
From the Tools menu, choose Options.
3
Select Capture as the schematic editor and close the
Options dialog box.
773
Chapter C
Importing Spice Models
Product Version 10.5
4
From the File menu, choose Export to Capture Part
Library.
5
Specify the location of the model library (.LIB) for which
you want the symbols to be created.
6
Specify the location of the part library (.OLB) to be
created and select OK.
7
A message box appears displaying status of part creation
process. Select OK to close the message box.
Note: Any errors or warning messages that are
generated during the part creation, are saved in a log file
named <library_name>.err. Referring to the
contents of the .err file might be helpful, in cases where
part creating fails.
Creating symbol for a model
1
From the Tools menu, choose Options.
2
To enable part creation every time you save a model,
select the Always Create Part when Saving Model
check box.
3
Select Capture as the schematic editor.
4
Using the Save Part To group box, specify the library in
which the new part should be saved and close the
Options dialog box.
After making the modifications in the Options dialog box, a
symbol will be generated for the part every time you save the
774
PSpice User's Guide
Product Version 10.5
Generating Part Symbols
changes in your custom model. The generated symbol will
have the same name as that of the simulation model. The
name and location of the part library (.OLB) will be same as
that of the model library (.LIB).
Important
If the downloaded Spice model is of .SUBCKT type,
the Model Editor generates a rectangular symbol.
You can edit the Model Editor generated symbol
shapes. For more information, see Editing Model
Editor created symbols.
Using symbols from an existing symbol library
Instead of creating a new symbol from scratch, you can use a
symbol from an existing part library, and associate it with the
downloaded model. Using symbols from an existing library
involves following steps:
■
■
Copying the symbol
❑
Copying parts within the same library
❑
Copying a part to another library
Modifying the IMPLEMENTATION property
Before you can use a part symbol from an existing OLB, you
need to know the type of simulation model attached with the
source part. If the original part symbol is attached to a device
characteristic curves-based PSpice model, you only need to
modify the implementation property. In case the original part
symbol is attached to a template-based PSpice model, you
will need to add the IMPLEMENTATION and the
PSPICETEMPLATE property to the copied model.
Caution
It is recommended that unless you are very
comfortable with different types of simulation
models supported by PSpice, you should avoid
situations where PSPICETEMPLATE property
needs to be changed. You can either create
PSpice User's Guide
775
Chapter C
Importing Spice Models
Product Version 10.5
symbols using the Model Editor or if you want to
copy a symbol, select a symbol of same type and
change the IMPLEMENTATION property.
Copying the symbol
Before you copy the part symbol, it is recommended that you
create a custom Userlib folder to store your custom symbol
and model libraries. Create a sub folder in the pspice folder
called Userlib to store your custom libraries.
−
To create a new library in Capture, from the File menu,
choose New and then from the submenu, choose Library.
Copying parts within the same library
Capture does not allow direct copying and pasting of a part in
the same library. Therefore, you need to complete the
following steps:
1
In Capture, open the symbol library from which you want
to copy the symbol. From the File menu, choose Open
and then choose Library.
2
Click on the part to be copied so that it becomes
highlighted.
3
From the Edit menu choose Copy.
4
Right-click on the part you just copied and select
Rename.
5
Type in the name of the new part and click OK.
6
From the Edit menu, choose Paste to paste the original
part back into the library.
Copying a part to another library
1
776
Open two part libraries in Capture. First, the source
library from which the part is to be copied and the second,
the destination library to which the model is to be copied.
From the File menu, choose Open | Library.
PSpice User's Guide
Product Version 10.5
Generating Part Symbols
2
In the Project Manager for the symbol library, position the
libraries in a way to enable dragging the part from one
library to another.
3
While holding down the Ctrl key, drag and drop the
required part from the source library to the destination
library.
Note: Alternatively, you can copy the desired part with
'Edit | Copy' and 'Edit | Paste' commands.
4
Right click on the part you just copied, select Rename,
and give the part the desired part name.
Modifying the IMPLEMENTATION property
If you have used existing part symbols, you must ensure that
the symbols you have copied and renamed point to the correct
model. The part to model referencing is done using the
Implementation property.
1
To edit the value of the IMPLEMENTATION property,
open the property editor by double clicking on the part.
Alternatively, right-click on the part and from the popup
menu choose Edit Properties.
2
In the Property Editor dialog box, ensure that the
Implementation Type is set to PSpice Model.
3
Change the value of the Implementation property to the
name specified in the model library (.LIB) file.
Note: In case IMPLEMENTATION property is not already
present, click New Row. In the Add New Row dialog
box, specify Name as Implementation and Value as
the name of the simulation model in the .LIB file.
Important
You need not specify any value in the
IMPLEMENTATION PATH field, because PSpice will
search the model only in the libraries that are
configured for the project. Model libraries will be
searched in the same sequence as listed in the
Library Files list box in the Libraries tab of the
simulation setting dialog box.
PSpice User's Guide
777
Chapter C
Importing Spice Models
Product Version 10.5
Adding PSPICETEMPLATE property
The PSPICE TEMPLATE property is required if you want to
simulate the part. This property defines the PSpice syntax
required for the netlisting the part. This property is not
required for parts based on PSpice provided templates. For
detailed information on PSPICETEMPLATE property, see
PSPICETEMPLATE on page 263.
Using Model Import wizard
If you are using Model Editor from release 10.5, you can use
the Model Import wizard either to generate a symbol for the
imported model or to associate an existing model to the
imported symbol.
Launching Model Import wizard
You can invoke Model Import wizard, using one of the
methods listed below.
■
Using File menu
a. From the File menu in Model Editor, choose Model
Import Wizard [Capture].
■
Using Tools menu
a. From the Tools menu, choose Options.
b. Select the Always Create Part When Saving
Model check box.
c. Select the Pick symbols manually check box.
d. Click OK.
Model Import wizard is launced whenever you save
the model.
Associating Model
If you launch Model Import wizard from the File menu, in the
first page of the wizard, you need to specify the path to the
778
PSpice User's Guide
Product Version 10.5
Configuring new model library
input simulation library as well as the location of the
destination symbol library and click Next.
Model Import wizard starts the process of associate a symbol
to the downloaded simulation model.
In the Associate/Replace Symbol page of the wizard, you can
view the symbol associated with the downloaded model and if
required, replace it with the symbol of your own choice.
1
Select the Replace Symbol button.
Note: If no symbol was associated to the model by the
Model Import wizard, use the Associate Symbol button
that is available instead of the Replace Symbol button.
2
In the Select Matching page of the wizard, specify the
path to the symbol library containing the symbol to be
associated with the downloaded model.
3
From the Matching Symbols list, select the symbol that
you want to associate with the downloaded model and
click the Save Symbol button.
4
In the Associate/Replace Symbol page, the selected
symbol name appears against the downloaded model
name. Click Finish to save your changes to the symbol
library.
When you use the Model Import wizard to generate or
associate symbols to a downloaded model, all the required
properties, such as IMPLEMENTATION TYPE,
IMPLEMENTATION, and PSPICETEMPLATE, are also
updated. Therefore, you need not modify these properties
manually.
Configuring new model library
After you have generated the part library for a new/customized
model library, you need to make the model library available to
the design. To ensure this you need to add the model library
containing your custom simulation models to the project
simulation profile.
1
PSpice User's Guide
In Capture, open your Analog or Mixed-Circuit project.
779
Chapter C
Importing Spice Models
Product Version 10.5
2
From the PSpice menu choose Edit Simulation Profile.
3
Select the Configuration Files tab.
4
In the Category list box, select Library.
5
In the Filename text box, specify the location of the model
library.
6
To make the library available to all designs, click Add as
Global. If you want the library to be used only in the
current design, select Add to Design and close the
Simulation Settings dialog box.
Note: Instead of editing a simulation profile, you can also
create a new simulation profile. To do this, choose New
Simulation Profile from the PSpice menu in Capture.
780
PSpice User's Guide
Product Version 10.5
Editing Model Editor created symbols
Editing Model Editor created symbols
Depending on the model definition, different symbol shapes
are generated by the Model Editor. Regular symbol shapes
are generated for the standard PSpice primitive models that
are defined using the .MODEL statement. For devices based on
a more complicated subcircuit model definition, .SUBCKT, a
generic rectangle is created that interfaces with the subcircuit
model.
For example, if the downloaded simulation model is an
OPAMP model defined using a.SUBCKT statement, the
symbol generated by the Model Editor will be a generic
rectangular graphic with pins attached.
In such cases, you can edit the symbol created by the Model
Editor. This section demonstrates the steps for editing the
symbol generated using the Model Editor for an OPAMP
simulation model LF442A.MOD, downloaded from the
National Semiconductor’s web site. LF442A is a Dual Low
Power JFET Input Operational Amplifier. After you download
the simulation model, use the Model Editor to generate the
part symbol, as explained in the Generating Part Symbols
section.
1
After the symbol generation is complete, open the Model
Editor created symbol library in Capture.
e. Launch Capture. From the Start menu choose
Programs > Release OrCAD 10.0 > Capture.
f. From the File menu in Capture, choose Open >
Library.
2
PSpice User's Guide
Double click on the part for which the symbol is to be
modified.
781
Chapter C
Importing Spice Models
Product Version 10.5
The part symbol appears as shown below.
Instead of a regular triangular graphic, a rectangular
graphic is generated. The numbers inside the rectangle
are the pin names and the numbers outside the rectangle
represent pin numbers.
You will now edit the Model Editor generated symbol to
have a triangular shape.
3
Delete the shape within the dotted line.
4
Redraw the required figure.
For an OPAMP the required figure is a triangle.
a. From the Place menu, choose Line.
b. Draw a triangle as shown below.
Note: For detailed procedure see the Editing part
graphics section in Chapter 5, Creating parts for
models of the PSpice User Guide.
5
782
Reposition the pins such that the inverting and the non
inverting inputs are on the top left and bottom left of the
modified symbol. The positive power supply should be on
the top and the negative power supply at the bottom. The
PSpice User's Guide
Product Version 10.5
Editing Model Editor created symbols
Output pin should be placed to the right of the modified
symbol.
For repositioning pins you need to refer to the pin names
as well as the model definition. This is because the pin
names are used for model definition.
The relevant section from the model definition for LF442A
relating pin names is shown below:
Reposition the OPAMP pins as shown in the figure below:
Using the line tool, draw lines to join pin numbers 3 and 4
to the modified symbol.
6
PSpice User's Guide
You can also change the pin numbers and the pin type
using the Pin Properties dialog box.
783
Chapter C
Importing Spice Models
Product Version 10.5
Important
Do not change the pin name because pin names are
used in the model library (.lib) file for model
definition.
7
After modifying the symbol as per your specifications,
save the symbol and the part library.
You can now use the modified symbol in your design.
For more details on creating custom parts see, Editing part
graphics and Basing new parts on a custom set of parts in
Chapter 5, Creating parts for models.
784
PSpice User's Guide
PSpice SLPS Interface
D
What is PSpice SLPS Interface?
PSpice SLPS Interface is an interface tool that links PSpice to
the MATLAB modeling tool and also to Simulink system
simulator, provided by The Mathworks. This interface tool has
been developed in partnership with Cybernet Systems Co Ltd.
PSpice is a SPICE-based simulator used for simulating
electrical and electronic circuits, and The Mathworks tools are
used for system designing. PSpice SLPS interface integrates
these two simulators to provide a simulation flow that can be
used to design any kind of system with electronic
sub-systems.
Circuits with PSpice models can now be included in system
model. PSpice SLPS Interface allows users to substitute
electronic blocks in PSpice, while the rest of the design is
simulated using MATLAB or Simulink. As a result, you can
now use a single prototype to co-simulate the electrical and
mechanical systems. Co-simulation environment allows to
simulate whole system with more realistic element models
before trial manufacturing.
To go through the step by step instructions for using PSpice
SLPS Interface, see PSpice SLPS Interface User's Guide.
You can download this user guide from
http://www.cybernet.co.jp/slps/download.
PSpice User's Guide
785
Chapter D
PSpice SLPS Interface
Product Version 10.5
How to get PSpice SLPS Interface?
You can download the latest version of PSpice SLPS Interface
from http://www.cybernet.co.jp/slps/download.
To be able to use PSpice SLPS Interface, you need to acquire
SLPS license from Cadence, and should have the following
combination of The Mathworks and OrCAD products installed
on your system:
■
■
The Mathworks products (R13 or higher)
❑
MATLAB 6.5
❑
Simulink 5.0
OrCAD products (R10.0 Service Pack 2 or higher)
❑
R10.0 SP 2 Capture (CIS)
❑
R10.0 SP 2 PSpice A/D
Instead of above two products you can also install one of
the following Unison products.
786
❑
R10.0 Unison EE
❑
R10.0 Unison Ultra
PSpice User's Guide
Index
.ALS file, 388
.CIR files, 49
.DAT files, 53, 646, 658, 663
.INC files, 52, 202, 204
.LIB files, 51
.mcp file, 502
.NET files, 48
.OUT files, 53, 75
.PRB files, 630–632
.STL files, 51, 477
.STM files, 51
A
A/D Basics, 24
A/D Lite, PSpice product, 26, 30
ABM
ABM (analog behavioral modeling),
275–326
ABM part templates, 280
ABM.OLB, 277
basic components, 281, 284
basic controlled sources, 326
behavioral, 120
cautions and recommendations for
simulation, 320
Chebyshev filters, 281, 286, 324
control system parts, 281
PSpice User's Guide
custom parts, 326
expression parts, 283, 299
frequency domain device models, 315
frequency domain parts, 315, 321
frequency table parts, 307, 317, 325
instantaneous models, 309, 320
integrators and differentiators, 282, 290
Laplace transform, 282, 296, 307, 315,
322
limiters, 281, 285
math functions, 282, 299
mathematical expressions, 307
overview, 276
placing and specifying ABM parts, 278
PSpice A/D-equivalent parts, 307–308
signal names, 275
simulation accuracy, 325
syntax, 308
table look-up, 282, 291, 307, 313
triode modeling example, 303
AC stimulus property, 441
AC sweep analysis, 372, 438–447
about, 438
displaying simulation results, 90
example, 88, 444
introduction, 40
noise analysis, 372, 448–456
setup, 88, 438, 442
787
Index
stimulus, 439
treatment of nonlinear devices, 446
accelerator keys, see online PSpice Help
ACMAG stimulus property, 441
ACPHASE stimulus property, 441
Advanced Analog Options dialog box, 383
advanced analysis libraries, 38, 113
algorithms
see also models
analog and digital in PSpice A/D, 24
built in to PSpice, 151
Newton-Raphson, 752
solution algorithms, 383
ambiguity
cumulative hazard, 572
analog behavioral modeling, see ABM
analog parts, see parts
analyses
AC sweep, 88, 372, 438–447
bias point, 73, 372, 429–430
DC sensitivity, 372, 434
DC sweep, 76, 372, 420–427
digital worst-case timing, 594–608
Fourier, 372, 493
frequency response, 372
Monte Carlo, 373, 506–527
noise, 372, 448–456
overview, 40, 372
parametric, 93, 373, 457–458, 466
performance analysis, 101, 461
sensitivity/worst-case, 373, 528–538
setup, 373
small-signal DC transfer, 372, 431–433
statistical, see Monte Carlo or sensitivity
/ worst-case analyses
temperature, 373, 467–468
transient, 83, 372, 471–494
types, 40–44, 372
appending
waveform data files in Probe, 614, 658
approximation, problems, 755
arithmetic functions for Probe, 700
ASCII waveform data, 663
788
Product Version 10.5
AtoD interface, see mixed analog/digital
circuits
B
Basics, overview, 25
bias point
save/load, 746
bias point detail analysis, 429–430
example, 73
introduction, 40
bipolar transistors
see also parts
Bode plot
example, 91
using plot window templates, 41, 633
Boolean expression example, 362
C
capacitors, see parts
Capture
see also OrCAD Capture User’s Guide
Add Library button, 65
advanced markers, 90
bias point analysis setup, 429
Create PSpice Project dialog box, 64
Parts Spreadsheet, 70
Place Part dialog box, 65
Property Editor, 70
simulate a circuit from, 74
starting Model Editor from, 178
starting Stimulus Editor from, 478
Model Import Wizard, 240
causal, 294, 323
charge storage nets, 347
circuit file (.CIR), 49
simulating multiple circuits, 395
color printing, waveforms, 617
COMMANDn stimulus property (digital),
554
Common Simulation Data Format (CSDF),
663
components, see parts, 117
PSpice User's Guide
Product Version 10.5
configuring, 620
model libraries, 202–210
overview, 52
stimulus files, 477
strength scale, 350
waveform display, 622
waveform update intervals, 624
connection, node, 145
continuous equations
problems, 754
convergence hazard, 572
convergence hazard, digital worst-case
timing, 599
convergence problems
approximations, 755
continuous equations, 754
derivatives, 754
diagnostics, 756
Newton-Raphson requirements, 752
Create Subcircuit Format Netlist command,
160, 196
Creating
Advanced Analysis-enabled Pspice
models, 171
parameterized models, 171
Creating Capture parts, 238
Creating models
based on device characteristic curves,
166
based on PSpice templates, 171
creating parts
interactive mode, 240
critical hazard, digital worst-case timing,
600
CSDF, Common Simulation Data Format,
663
cursors, waveform analysis, 682
custom part creation for models, 254
using the Model Editor, 237
D
data collection, limiting, 647
data collection, limiting file size, 647
PSpice User's Guide
Index
DC analyses
displaying simulation results, 78
see also DC sweep analysis, bias point
detail analysis, small-signal DC
transfer analysis, DC sensitivity
analysis
DC sensitivity analysis, 372, 434
introduction, 40
DC stimulus property, 424
DC sweep analysis, 372, 420–427
about, 421
curve families, 426
example, 76
introduction, 40
nested, 424
setting up, 76
stimulus, 423
DELAY stimulus property (digital), 552
derivative
problems, 754
design
preparing for simulation, 46, 108
DESIGN_NAME-ROOT_SCHEMATIC_NA
ME.NET, 48
DESIGN_NAME-ROOT_SCHEMATIC_NA
ME-PROFILE_NAME.SIM.CIR, 49
developer’s kit, PSpice (call Customer
Support), 29
Device Equations Developer’s Kit (call
Customer Support), 29
device noise, 449, 452
Device types
characteristic curves-based, 170
template-based, 173
device types
breakout parts, 119
E and G devices, 308
Model Editor, 170, 173
passive parts, 117
PSpice-equivalent parts, 307
three- and four-terminal, 381
devices, see parts or models
diagnostic problems, 756
789
Index
dialog box
Advanced Analog Options, 383
Arguments for Measurement
Evaluation, 714
Display Control (Probe), 630
Display Measurement Evaluation, 717
Measurements, 714
Simulation Message Summary, 687
Traces for Measurement Arguments,
715
DIG_GND stimulus property (digital), 553
DIG_PWR stimulus property (digital), 553
DIGDRVF (strengths), 351
DIGDRVZ (strengths), 351
DIGERRDEFAULT (simulation option), 574
DIGERRLIMIT (simulation option), 574
DIGIOLVL (simulation option), 337
digital device modeling, 329–366
digital primitives list, ??–334
digital primitives syntax, 334
example "U" device declaration, 337
functional behavior, 331
inertial delay, 343
input/output characteristics, 346–357
AtoD and DtoA subcircuits, 353
charge storage on nets, 352
configuring the strength scale, 350
controlling overdrive, 352
defining output strengths, 350
I/O model, 346
I/O model parameters, 348
internal delay functions, 343
overview, 330
propagation delay calculation, 342
timing characteristics, 339–344
timing model, 339
unspecified propagation delays
unspecified timing constraints, 341
transport delay, 344
digital primitives
see also parts
input (N device), 354
output (O device), 354
790
Product Version 10.5
propagation delays, see timing model
syntax, 334
timing model, see timing model
digital signals, see traces
digital simulation, ??–575
adding digital trace expressions, 565
ambiguity convergence hazard, 570
analyzing results, 563
controlling warning messages, 571
displaying waveforms, 563
hazard messages, 572
inertial delay, 343
initialization options, 562
internal delay functions, 343
messages, 571
output control options, 573
plotting results, 564, 566
propagation delays, see timing model
severity level messages, 574
states, 350, 541
strengths, 350
timing characteristics, 339–344
timing model, 339
timing constraints, unspecified, 341
timing violation messages, 571
timing violations and hazards, 569
transport delay, 344
vector file, 743
waveform display, 669, 700, 703
worst-case timing, 594
digital worst-case timing, 594–608
ambiguity in the feedback path, 602
ambiguity region, 596
compared to analog worst-case, 595
constraint checkers, 604
constraints of applied stimulus, 594
convergence hazard, 572, 599
convergence hazard example, 599
critical hazard, 600
critical hazard example, 600
cumulative ambiguity hazard, 572, 601
cumulative ambiguity hazard examples,
601
PSpice User's Guide
Product Version 10.5
glitch suppression, 573
glitch suppression due to inertial delay,
605
glitch suppression examples, 605
methodology, 606
MIN/MAX delay spread, 598
mixed-signal and all-digital circuits, 595
no combined analog/digital worst-case
analysis, 595
pattern-dependent mechanism, 594
reconvergence hazard, 603
reconvergence hazard example, 603
setup, 596
timing ambiguity, 596
timing ambiguity examples, 597–598
timing hazard example, 599
DIGMNTYMX (simulation option), 596
DIGMNTYSCALE (simulation option), 340
DIGOVRDRV (simulation option), 352
DIGPOWER (I/O model), 347
DIGTYMXSCALE (simulation option), 340
diodes, see parts
Display Control dialog box, 630
display modes
alternate (plots only), 615
default (standard), 615
documentation
conventions, 20
online help, 21
online PSpice Library List, 116
example entries, 115
online PSpice Quick Reference, 23
online PSpice Reference Guide, 22
online PSpice User’s Guide, 21
documentaton
OrCAD Capture User’s Guide, 23
DRVH (I/O model parameter), 591
DRVH (I/O model), 347, 351
DRVL (I/O model parameter), 591
DRVL (I/O model), 347, 351
DRVZ (I/O model), 347
DtoA interface, see mixed analog/digital
circuits
PSpice User's Guide
Index
E
examples and tutorials, 601
"U" device declarations, 337
ABM expression part examples, 300–
303
AC sweep analysis, 88, 444
analog waveform analysis, 663
bias point detail analysis, 73
Chebyshev filter and Monte Carlo
analysis, 521
Chebyshev filter parts, 287–289
circuit creation, 64
creating a digital model, 358, 366–368
creating AA enabled PSpice model, 187
creating parts using the Model Editor,
246
DC sweep analysis, 76
digital worst-case timing ambiguity,
597–598
digital worst-case timing reconvergence
hazard, 603
EMULT part example, 311
EVALUE part example, 310
Fourier analysis, 666
frequency response vs. arbitrary
parameter, 464
FTABLE part example, 293
glitch suppression, 605
glitch suppression,digital worst-case
timing, 605
GMULT part example, 312
GVALUE part example, 311
hysteresis curves with transient
analysis, 492
Laplace transform, 316
Laplace transform part examples, 296–
298
measurement definition example, 722
measurement definition syntax, 734–
735
measurement expressions, 714–720
mixed analog/digital waveform analysis,
669
791
Index
mixed signal oscillator circuit, 670–673
modeling a triode (ABM), 303
Monte Carlo analysis, 512
noise analysis, 453
parametric analysis, 93, 459, 464
performance analysis, 101, 459
PSPICETEMPLATE part property, 267–
271
simulations, 63–103
temperature analysis, 665
transient analysis, 83, 665
using the Model Editor, 180–187, 195
using the Stimulus Editor, 479
worst-case analysis, 531
worst-case timing, digital, see digital
worst-case timing examples
export
waveform data, 681
expressions, 124
see also parameters
ABM, 307
functions, 126–129
specifying, 124
waveform analysis, 700
F
file
Monte Carlo Parameter (.mcp), 502
files
appending waveform files, 658
circuit (.CIR), 49
configuring, 52
generated by Capture, 48
generated by PSpice, 53
include (.INC), 52, 202, 204
limiting data collection, 647
limiting waveform file size, 646, 650, 663
model library (.LIB), 50
netlist (.NET), 48
output (.OUT), 53
Probe windows (.PRB), 630–632
stimulus (.STM, .STL), 51, 477
user-configurable, 50
792
Product Version 10.5
waveform (.DAT), 53, 646, 658
with simulation results, 53
flat netlist
creating, 388
overview, 385
flicker noise, 452
flip-flops
initialization options, 562
floating node, 146
FORMAT stimulus property (digital), 553
Fourier analysis, 372, 493
displaying Fourier transform, 666
example, 666
FFT (Fast Fourier Transform), 494
fundamental Fourier period, 494
introduction, 42
print step, 494
FREQUENCY output variable, 694
functions
waveform analysis, 700
G
GaAsFETs, see parts
glitch suppression, 573, 605
global parameters, 121
goal functions, see measurements
graph, see plot, Probe window, traces,
waveform analysis
ground
see also parts, 111
missing, 146
missing DC path to, 146
group delay (output variable AC suffix), 695
H
hardware requirements for PSpice
software, 30
help online, 21
hierarchical netlist
creating, 388
customizing, 390
no cross-probing from a subcircuit, 387
PSpice User's Guide
Product Version 10.5
overview, 386
SUBPARAM part, 387
histograms, 521
how to use the user’s guide, 20
hysteresis curves, 492
I
I/O model, 334–335, 346, 579
and switching times (TSW), 348
DIGPOWER, 347
DRVH, 347
DRVL, 347
DRVZ, 347
INLD, 346
INR, 347
OUTLD, 346
parameter summary, 348
TPWRT, 343, 347
TSTOREMN, 347
IC (property), 750
icon
in Simulation Manager, 410
push pin, 616
imaginary part (output variable AC suffix),
695
importing traces, 659
include files (.INC)
configuring, 52, 202
with model definitions, 204
inductor coupling, see parts
inductors
see also parts
inertial delay, 343
initial conditions, 746, 750
INLD (I/O model), 346
input noise, total, 452
INR (I/O model), 347
instance models
and the Model Editor, 177
changing model references, 199
editing, 179
reusing, 200
saving for global use, 179
PSpice User's Guide
Index
interface subcircuits, 353, 578, 591
and I/O models, 335, 579
and power supplies, 578
CAPACITANCE, 354
customized, 353
DRVH, 354
DRVL, 354
IO_LEVEL, 334
N device (digital input), 354
O device (digital output), 354
syntax, 354
IO_LEVEL
interface subcircuit parameter, 334
part property, 272
stimulus property (digital), 553
IO_MODEL stimulus property (digital), 553
J
JFETs, see parts
K
keyboard shortcuts, see online PSpice Help
L
Laplace transforms and non-causality, 323
large data files, 650
displaying fewer data points, 651
displaying partial trace, 651
threshold, 656
viewing options, 650
latches
initialization options, 562
libraries
see also model libraries
adding to design, 65
changing from design to global, 206
changing from profile to design, 206
changing from profile to global, 206
configuring, 202
handling duplicate model names, 205
model, 152
793
Index
package, 52
parts (.OLB), 52
parts and models list
path name to PSpice part libraries, 65
search order, 204, 208
searching for models, 203
library list (separate online document), 22,
116
example entries, 115
Lite, PSpice A/D product, 26, 30
loading delay, 342
M
macromodel (subcircuit), 51
magnitude (output variable AC suffix), 695
markers, 646
displaying traces, 78
for limiting waveform data file size, 646
for waveform display, 626
placing on schematic, 628
plot window template markers, 643
measurement, 461
expressions, 710
in performance analysis, 463
overview, 710
results, 713
single data point, 463
strategy, 711
measurement definition
creating custom definitions, 721
example, 722
list, 718
selecting and evaluating, 712
syntax, 725
writing a new definition, 722
measurement expression
composing, 712
creating, 712
list of definitions, 718
measurement definition, 712
output variables, 712
setup, 712
Simulation Results view, 712
794
Product Version 10.5
value in PSpice, 713
viewing in PSpice, 713
menu and shortcuts reference, 23
messages, simulation, 571
mixed analog/digital circuits, 358, 372
I/O models, 579
interconnecting analog and digital parts,
578
interface subcircuits, 272, 578
IO_LEVEL property, 272
power supplies, 578, 591
waveform display, 669, 700, 703
MNTYMXDLY
part property, 273
timing model parameter, 334
model and part libraries, see library list
Model Editor
about, 47, 193
analyzing model parameter effects, 168
changing
.MODEL definitions, 194
.SUBCKT definitions, 194
model names, 194
creating AA enabled PSpice model, 187
creating parts, 246
creating parts for models, 175, 237
custom, 254
example, 195
fitting models, 169
from the schematic page editor, 177
starting stand-alone, 165
supported device types, 170, 173
testing and verifying models, 167
tutorial, 180–187
using data sheet information, 168
viewing performance curves, 170
ways to use, 164
model libraries
about, 50, 152
adding to the configuration, 205
analog list of, 142
configurating, 153
configuring, 52, 144, 202, 204
PSpice User's Guide
Product Version 10.5
digital list of, 143
directory search path, 210
duplicate model names, 205
for part creation, 235
global vs. design vs. profile, 153, 206
how PSpice searches them, 203
nested, 154
NOM.LIB, 155
preparing for part creation, 235
search order, 204, 208
model list, see library list
MODEL property, 151, 260
models
analog behavioral modeling (ABM),
275–326
built-in, 36
changing associations to parts, 199
creating parts for
custom, 254
using the Model Editor, 175, 237
creating with the Model Editor, 193
defined as
parameter sets, 151
subcircuits, 151, 196
digital device modeling, 329–366
digital I/O characteristics, 346–357
digital timing characteristics, 339–344
global vs. design vs. profile, 153
instance, 177, 199–200
organization, 152
preparing for part creation, 235
saving as design
using the Model Editor, 177
testing/verifying (Model Editor-created),
167
tools to create, 160
ways to create/edit, 161
Monte Carlo
History support, 498
reusing parameter values, 500
saving parameter values, 498
Monte Carlo analysis, 373, 506–527
collating functions, 504
PSpice User's Guide
Index
histograms, 521
introduction, 43
model parameter values reports, 497
output control, 497
tutorial, 512
using the Model Editor, 195
waveform reports, 503
with temperature analysis, 505
Monte Carlp Parameter (.mcp) file, 502
MOSFETs, see parts
multiple y-axes, waveform analysis, 463
N
netlist
creating flat, 388
creating hierarchical, 388
creating subcircuit format, 392
creating the netlist, 388
customizing hierarchical, 390
failure to netlist, 110
file (.NET), 48
flat, overview, 385
hierarchical, no subcircuit
cross-probing, 387
hierarchical, overview, 386
hierarchical, subcircuit limitations, 387
passing parameters to subcircuits, 386
PSPICETEMPLATE property, 386
subcircuit format, 392
templates, 386, 393
Newton-Raphson requirements, 752
node
connection, 145
floating, 146
interface, 578
noise analysis, 372, 448–456
about, 40, 449
device noise, 449
example, 453
flicker noise, 452
noise equations, 452
setup, 448, 450
shot noise, 452
795
Index
thermal noise, 452
total output and input noise, 449
units of measure, 453
viewing results, 453
viewing simulation results, 452
waveform analysis output variables, 452
noise units, 453
non AA enabled PSpice models, 155
non-causal, 293, 323
nonlinear devices
in AC sweep analysis, 446
NOOUTMSG (simulation option), 574
NOPRBMSG (simulation option), 574
O
OFFTIME stimulus property (digital), 553
online help, 21
online PSpice Advanced Analysis Library
List, 23
ONTIME stimulus property (digital), 553
on-top window display, 616
OPPVAL stimulus property (digital), 553
options
DIGERRDEFAULT, 574
DIGERRLIMIT, 574
DIGIOLVL, 337
DIGMNTYMX, 596
DIGMNTYSCALE, 340
DIGOVRDRV, 352
DIGTYMXSCALE, 340
NOOUTMSG, 574
NOPRBMSG, 574
RELTOL, 325
SOLVER, 383
OrCAD Capture, see Capture
OUTLD (I/O model), 346
output file (.OUT), 53
control parts, 739
messages, 571
negative current values, 75
tables and plots, 739
viewing from PSpice, 75
output noise, total, 452
796
Product Version 10.5
output variables, 376–382
arithmetic expressions, 700
digital signals and buses, 704
digital trace expression, 704
noise (waveform analysis), 452
selecting, 712
waveform analysis, 689, 703, 705
waveform analysis functions, 700
output window, 399
P
PARAM example, 460
Parameterized models, 157
parameterized parts, 38, 113
parameters
distribution, 39, 114
global, 121–123
interactive simulations, 400–408
optimizable, 38, 114
passing to subcircuits, 386
runtime, 400, 404–408
simulations, interactive, 400
smoke, 38, 114
SUBPARAM, 387
tolerance, 38–39, 114
parametric analysis, 373, 457–466
analyzing waveform families, 97
example, 93, 459, 464
frequency response vs. arbitrary
parameter, 464
introduction, 43, 459
minimum circuit requirements, 458
multi-run analysis, 459
performance analysis, 459–462, 465
setting up, 94
setting up analysis, 458
swept variables, 458
temperature analysis, 373, 467
transient analysis requirement, 458
parts
pins, 274
part and model libraries, see library list
part wizard
PSpice User's Guide
Product Version 10.5
using custom parts, 254
parts
attaching models to, 259
behavioral, 120
bipolar transistors, 119, 170, 173, 381,
698–699
breakout, 118
capacitors, 117, 119, 380
Chebyshev filters, 521
comparator, 170
controlled sources, 326
creating custom parts, 175
creating for models
custom parts, 254
using the Model Editor, 175, 237
creating new stimulus parts, 483
current source, 380
controlled, 307, 326
current-controlled, 380
DC current source, 133
voltage-controlled, 380
Darlington model transistors, 170
DC voltage source, 133
digital primitives, 331, 359
digital primitives list, ??–334
digital source, 133
diodes, 170, 173, 380, 698
editing graphics, 256
finding, 115
GaAsFETs, 119, 381, 697–698
grid spacing
graphics, 258
pins, 258
ground, 111
IGBTs, 119, 170, 173, 381, 698
imaginary part, 695
in library lists, 112
inductor coupling, 119
inductors, 119, 380
IO_LEVEL property, 272
JFETs, 119, 126–127, 136, 170, 173,
381, 697, 699
logic propagation delays, 560
PSpice User's Guide
Index
Lossy transmission line TLOSSY, 117
magnetic core, nonlinear, 171, 173
MNTYMXDLY property, 273
MODEL property, 260
models, 259
MOSFETs, 119, 381, 698–699
naming conventions, 114
non-simulation, 264
nonlinear magnetic core, 171, 173
opamp (operational amplifier), 170, 173
output control, 111, 739
PARAM, 122
passive, 117
pins, 145, 258, 270
power supply, 591
A/D interfaces, 133
analog, 133
custom CD4000, 585, 587
custom ECL, 585, 587
custom TTL, 585, 587
DC source, 133
default digital power supply
selection, 583
digital, 133, 585, 587
preparing model libraries for part
creation, 235
primitives, digital, 359
properties for simulation, 262
PSPICEDEFAULTNET property, 274
PSPICETEMPLATE property, 263
real part, 696
regulator, 170, 173
resistors, 117, 119, 380, 699
saving as global
using the Model Editor, 175, 237
simulation control, 111
simulation parts, 111
simulation properties, 232
stimulus, 111
switches, 699
current-controlled, 119, 380
voltage-controlled, 119, 380
transformers, 117, 119
797
Index
transmission lines, 117–118, 382, 698
unmodeled, 140
voltage comparator, 170
voltage reference, 170
voltage regulator, 170, 173
voltage source, 380
controlled, 307, 326
current-controlled, 380
voltage-controlled, 380
ways to create for models, 233
zero ground (SOURCE.OLB), 67
$G_DGND (reserved global net), 591
$G_DPWR (reserved global net), 591
ABMn and ABMn/I (ABM), 283, 300
ABS (ABM), 282, 299
AGND (ground), 146
ARCTAN (ABM), 282, 299
ATAN (ABM), 282, 299
BANDPASS (ABM), 281, 288
BANDREJ (ABM), 281, 289
BBREAK (GaAsFETs), 119
CBREAK (capacitors), 119
CD4000_PWR (digital power), 133
CD4000_PWR parts (power supply),
585
CONST (ABM), 281, 284
CONSTRAINT digital primitive, 120, 364
COS (ABM), 282, 299
CVAR (capacitors), 117
DBREAK (diodes), 119
DIFF (ABM), 281, 284
DIFFER (ABM), 282, 290
DIGCLOCK (digital stimulus), 138
DIGCLOCK digital stimulus, 543, 552
DIGIFPWR (digital power), 134
DIGIFPWR (power supply), 585, 591
DIGSTIM (digital stimulus), 138
DIGSTIM digital stimulus, 544
E (ABM controlled analog source), 326
ECL_100K_PWR (digital power), 134
ECL_100K_PWR (power supply), 585
ECL_10K_PWR (digital power), 134
ECL_10K_PWR (power supply), 585
798
Product Version 10.5
EFREQ (ABM), 307, 317
EGND (ground), 146
ELAPLACE (ABM), 307, 315
EMULT (ABM), 307, 311
ESUM (ABM), 307, 311
ETABLE (ABM), 307, 313
EVALUE (ABM), 307, 309–310
EXP (ABM), 282, 299
F (ABM controlled analog source), 326
FILESTIM (digital stimulus), 139, 554
FTABLE (ABM), 282, 292
G (ABM controlled analog source), 326
GAIN (ABM), 281, 284
GFREQ (ABM), 307, 317
GLAPLACE (ABM), 307, 315
GLIMIT (ABM), 281, 285
GMULT (ABM), 307, 311
GSUM (ABM), 307, 311
GTABLE (ABM), 307, 313
GVALUE (ABM), 307, 309–310
H (ABM controlled analog source), 326
HIPASS (ABM), 281, 288
IAC (AC stimulus), 440
ICn (initial condition), 748
ICn (initial conditions), 748
ICn (simulation control), 748
IDC (DC stimulus), 133, 423
INTEG (ABM), 282, 290
IPLOT (write current plot), 739
IPRINT (write current table), 741
ISRC (analog stimulus), 133, 138, 423,
440
ISTIM (transient stimulus), 136
JBREAK (JFETs), 119, 126–127, 136
K_LINEAR (transformer), 117
KBREAK (inductor coupling), 119
KCOUPLEn (coupled transmission
lines), 118
LAPLACE (ABM), 282, 296
LBREAK (inductors), 119
LIMIT (ABM), 281, 285
LOG (ABM), 282, 299
LOG10 (ABM), 282, 299
PSpice User's Guide
Product Version 10.5
LOGICEXP digital primitive, 120
LOGICEXP primitive, 358
LOPASS (ABM), 281, 287
MBREAK (MOSFETs), 119
MULT (ABM), 281, 284
NODESETn (initial bias point), 748
NODESETn (initial conditions), 748
PINDLY digital primitive, 120, 358
PRNTDGTLCHG (write digital state
changes), 742
PWR (ABM), 282, 299
PWRS (ABM), 282, 299
QBREAK (bipolar transistors), 119
RBREAK (resistors), 119
RVAR (resistor), 117
SBREAK (voltage-controlled switches),
119
SIN (ABM), 282, 299
SOFTLIM (ABM), 281, 285
SQRT (ABM), 282, 299
STIMn (digital stimulus), 138
STIMn digital stimulus, 553
SUM (ABM), 281, 284
T (ideal transmission line), 117
TABLE (ABM), 282, 291
TAN (ABM), 282, 299
TLOSSY (Lossy transmission line), 117
TnCOUPLEDx (coupled transmission
line), 118
VAC (AC stimulus), 135, 440
VDC (DC stimulus), 133, 135, 423
VECTOR (write digital vector file), 743
VEXP (transient stimulus), 136
VPLOTn (write voltage plot), 739
VPRINTn (write voltage table), 741
VPULSE (transient stimulus), 136
VPWL (transient stimulus), 136
VPWL_F_N_TIMES (transient
stimulus), 136
VPWL_F_RE_FOREVER (transient
stimulus), 136
VPWL_N_TIMES (transient stimulus),
136
PSpice User's Guide
Index
VPWL_RE_FOREVER (transient
stimulus), 136
VSFFM (transient stimulus), 136
VSIN (transient stimulus), 136
VSRC (analog stimulus), 133, 135, 138,
440
VSRC stimulus, 423
VSTIM (analog stimulus), 136
VSTIM (transient stimulus), 136
VSTIM stimulus part, 84
WATCH1 (view output variable), 738
WBREAK (current-controlled switches),
119
XFRM_LINEAR (transformer), 117
XFRM_NONLINEAR (transformer), 119
ZBREAK (IGBTs), 119
parts list, see library list
performance analysis, 459
example, 101
measurements, 461
performance package solution algorithms,
383
phase (output variable AC suffix), 695
piecewise linear (PWL) stimulus, 479, 484
pins, see parts
plot window template
copying, 639
creating, 633
deleting, 639
loading, 643
modifying, 637
placing markers in Capture, 643
restoring, 640
viewing properties of, 641
plots
see also Probe windows, waveform
analysis, traces, markers, plot
window templates
analog area, 613
arithmetic expressions for digital traces,
703
arithmetic functions for traces, 700
buses, adding, 566
799
Index
color, 617
cursors, 682
digital area, 613
digital traces, adding, 564
export data, 681
sizing, 676
templates, 633
waveform analysis, 613
y-axes, 671
power supplies, see parts, power supply
printing
in color, 617
Probe windows
see also plots, waveform analysis, plot
window templates
.PRB files, 630–632
arithmetic expressions for digital traces,
703
arithmetic functions for traces, 700
buses, adding, 566
color, 617
configure waveform view
digital traces, adding, 564
display control, 630
displaying on the schematic page, 616
exporting data, 681
making visible at all times, 616
managing multiple windows, 615
multiple y-axes, 671
noise analysis, 452
plot update methods, 678
plots, 613
printing Probe windows, 615
reusing with different simulations, 630
saving window contents, 630
scrolling, 676
setting colors, 617
sizing plots, 676
tabulating trace data values, 681
traces, displaying, 78
using cursors, 682–686
y-axes, 671
zoom regions, 674
800
Product Version 10.5
probes, see markers
PROFILE_NAME.CIR, 49
propagation delay, see timing model
PSpice models, 155
Pspice online help, 21
PSpice products
Device Equations Developer’s Kit
(DEDK), 29
evaluation version (PSpice A/D Lite), 26,
30
feature comparison, 26
minimum hardware requirements, 30
PSpice (analog circuits only), 25
PSpice A/D, 24, 36
PSpice A/D Basics, 25
PSpice A/D Lite, 26, 30
student version (PSpice A/D Lite), 26,
30
using with other programs, 46
PSpice SLPS Interface
documentation, 785
download, 786
overview, 785
PSPICE.INI file, editing, 617
PSPICEDEFAULTNET property, 274
PSPICETEMPLATE part property, 263–
271
examples, 267–271
importance in netlist, 386
naming conventions, 265
pin callout in subcircuits, 271
regular characters, 264
required for simulation, 386
special characters, 266
syntax, 264
push pin button, 616
PWL (piecewise linear) stimulus, 479, 484
Q
quick reference card (separate online
document), 23
PSpice User's Guide
Product Version 10.5
R
real part (output variable AC suffix), 696
Reference Guide (separate online
document), 22
regular PSpice models, 155
RELTOL (simulation option), 325
resistors, see parts
ROOT_SCHEMATIC_NAME.NET, 48
run data, see traces, waveform analysis,
output file, output variables, and
simulation results
RunFor text box (transient analysis), 402
runtime parameters
changing original values, 405
list of, 404
SCHEDULE expression syntax, 405–
406
scheduling changes to, 406
S
saving data
as ASCII text, 663
in the CSDF, 663
SCHEDULE (expression), 406
schematic
assign names to off-page connectors,
70
assign names to parts, 70
assign net names, 69
change part values (numbers), 71
connect parts, 68
create a new PSpice project, 64
label nets, 69
label off-page connectors, 70
move text associated with a part, 66
place a ground part, (SOURCE.OLB),
67
place a part, 65–66
place a voltage source, 65
place off-page connectors, 67
place the zero ground part, 67
place wires, 68
PSpice User's Guide
Index
rotate a part, 67
SOURCE.OLB ’0’ part (ground), 67
zero ground (GND) part, 67
schematic page editor, see Capture
scrolling, Probe windows, 676
shortcut keys, see online PSpice Help
shot noise, 452
simulation
about, 36
algorithm choices (SOLVER), 383
analysis
setup, 373
simulation profile, 373
types, 372
analysis window, 399
batch jobs, 395
bias point, 746
devices window, 399
digital, see digital simulation, 539
example
AC sweep analysis, 88
bias point analysis, 73
circuit creation, 64
DC sweep analysis, 76
parametric analysis, 93
performance analysis, 101
transient analysis, 83
failure to start, 110
hazard messages, 572
initial conditions, 746, 750
interactive, 400
interrupt and change parameters, 404
management, 409–418
messages, 399, 571
multiple circuit files, 395
multiple setups in one circuit file, 395
output file (.OUT), 75
part properties, 262–274
IO_LEVEL, 272
MNTYMXDLY, 273
PSPICEDEFAULTNET, 274
PSPICETEMPLATE, 263
pauses vs. stops, 401
801
Index
results
files, 53
output file, 737–744
using markers, 578
viewing, 415
waveforms, 563–568, 611–668
runtime parameters, 400, 404–408
scheduling parameter changes, 406
scheduling runtime parameter changes,
406
setup checklist, 108
solution algorithms (SOLVER), 383
starting, 385
starting from Capture, 394
starting outside of Capture, 394
status window, 396
timing violation messages, 571
troubleshooting checklist, 110
variable values log (Analysis window),
399
watch variable window, 399
Simulation Manager, 409–418
accessing it, 410
adding a simulation to the queue, 414
attaching PSpice to a simulation, 415
error handling, 413
functionality vs. PSpice product, 412
icon explanations, 410
job status explanations, 410–412
launching from the Start menu, 410
multiple simulations, setting up, 413
overview, 409
setting options, 415
starting, stopping, pausing simulations,
414
simulation models, 155
Simulation Settings dialog box
AC sweep/noise analysis, 89
bias point analysis, 73
DC sweep analysis, 76
parametric analysis, 95
transient (time domain) analysis, 86
802
Product Version 10.5
small-signal DC transfer analysis, 40, 372,
431–433
smoke
adding smoke information, 212
BJT, 220
Darlington Transistor, 229
diode, 219
IGBT, 222
JFET, 223
MOSFET, 226
OPAMP, 224
parameters, 218
Voltage Regulator, 228
solution algorithms (SOLVER), 383
SOLVER, 383
standard PSpice libraries, 37, 112
STARTVAL stimulus property (digital), 553
states, digital, 350, 541
statistical analyses, see Monte Carlo or
sensitivity / worst-case analyses
STIMTYPE property, 483
Stimulus Editor, 476–487
about, 46, 476
adjusting trace scale settings, 478
configuring stimulus files, 477
creating new stimulus parts, 483
defining analog stimuli, 136
defining digital inputs, 544
defining stimuli, 478
deleting traces (from graph), 485
editing a stimulus, 484
example, 84, 481
manual stimulus configuration, 485–487
PWL stimulus example, 479
removing traces (from file), 485
starting from outside of Capture, 485
starting in Capture, 478
stimulus files, 477
stimulus files
configuring, 52, 202, 477
stimulus generation, 474
manually configuring, 485
stimulus, adding
PSpice User's Guide
Product Version 10.5
AC sweep, 439
bus transitions (digital), 547
clock transitions (digital), 546
DC sweep, 423
for multiple analysis types, 137
loops (digital), 551
signal transitions (digital), 544
time-domain voltage, 83
transient (analog/mixed-signal), 474
transient (digital), 543
subcircuits, 151
analog/digital interface, 578
creating .SUBCKT definitions from
designs, 160
creating .SUBCKT definitions from
schematics, 196
netlist, 51, 392
no Probe markers in hierarchical netlist,
387
passing parameters to, SUBPARAM,
386
tools to create, 160
ways to create/edit, 161
see also models
SUBPARAM part, 387
switches
see also parts
syntax
ABM, 308
digital primitives, 334
measurement definition, 725
comments, 726
example, 734–735
marked point expressions, 727
names, 726
search command, 728
PSPICETEMPLATE, 264
SCHEDULE expression, 406
see also online Reference Guide
T
temperature analysis, 373, 467–468
default temperature, 468
PSpice User's Guide
Index
example, 665
introduction, 43, 468
setting up analysis, 467
with statistical analyses, 505
template
ABM parts, 280
netlisting, 386
part editor, 308, 312
plot window, 633–645
TEMPLATE property
and non-simulation parts, 264
template-based PSpice models, 157
test node mapping, 218
test vector file, 743
thermal noise, 452
TIME (Probe output variable), 694
time domain analysis, see transient analysis
TIMESTEP stimulus property (digital), 554
timing model, 334–335, 339
hold times (TH), 339
inertial delay, 343
loading delay, 342
propagation delays, 339, 560
calculation, 342
DIGMNTYSCALE, 340
DIGTYMXSCALE, 340
MNTYMXDLY, 273, 334
unspecified, 340
pulse widths (TW), 339
setup times (TSU), 339
switching times (TSW), 339
transport delay, 344
unspecified timing constraints, 341
timing violations and hazards
convergence, 572
cumulative ambiguity, 572
persistent hazards, 569
total noise, 449
TPWRT (I/O model), 343, 347
trace color schemes, 620
traces
see also output variables, plots, Probe
windows, and waveform analysis
803
Index
adding, 53, 78, 661, 690
appending, 658
arithmetic expressions, 700, 703
deleting from graph, 485
direct manipulation, 674
displaying, 78, 86
importing, 659
markers, 646
output variables, 689
placing a cursor on, 80
removing from file, 485
source data for a specific trace, 662
transformers
see also parts
transient analysis, 372, 471–494
analog, 472–494
bias point solution, 757
convergence problems, 752
digital, 372, 558
example, 83–87, 665
extending runtime, 401–403
Fourier analysis, 372
FTABLE DELAY property, 293
hysteresis curves, 492
internal time steps, 490
introduction, 42, 472
Maximum Time Step, 490
minimum requirements, 472
pausing at TSTOP, 402
print step, 490
response, 487–489
RunFor text box, 402
runtime parameters, 406
setting up, 85, 472, 487
Stimulus Editor, 476
stimulus generation, 474
switching circuits, 491
TIME (sweep variable), 694
time step analog vs. digital, 490
transient (time) response, 487–489
TSTOP, 401–402
transistors
see parts, bipolar transistors
804
Product Version 10.5
see parts, GaAsFETs
see parts, JFETs
see parts, MOSFETs
transmission lines, see parts
transport delay, 344
triode example, 303
troubleshooting
checklist, 110
missing DC path to ground, 146
missing ground, 146
performance analysis, 463
unconfigured libraries and files, 144
unmodeled parts, 140
unmodeled pins, 145
TSTOP, 401
extending a transient analysis, 402–403
TSTOREMN (I/O model), 347
TTL, 591
U
unmodeled
parts, 140
pins, 145
V
vector file, 743
voltage sources
negative current values, 75
see also parts
W
waveform analysis
about, 45
add markers in Capture, 90
configuring update intervals, 624
configuring waveform view, 622
cursors, 682
digital display name, 705
digital signals and buses, 704
displaying simulation results, 78, 90
PSpice User's Guide
Product Version 10.5
expressions,arithmetic expressions,
700
functions, 700
hysteresis curves, 492
interacting with waveform during
simulation, 625
limiting waveform data file size, 646
markers, 626
messages, 571
monitor results during simulation, 623
multiple y-axes, 463
output variables, 689, 703
for noise, 452
overview, 612
performance analysis, 101, 459
placing a cursor on a trace, 80
plot, 613
printing Probe windows, 615
setting colors, 617
traces
adding, 53, 78, 564, 661, 690
deleting from graph, 485
displaying, 674
source data for a specific trace, 662
tabulating data values, 681
using output variables, 689
viewing waveform of paused simulation,
626
waveform data file formats, 53, 663
waveform families, 97, 426
y-axes, 671
WIDTH stimulus property (digital), 553
worst-case analysis, 373, 528–538
collating functions, 504
example, 531
hints, 535
introduction, 43
model parameter values reports, 497
output control, 497
overview, 528
timing, digital, 594–608
waveform reports, 503
with temperature analysis, 505
PSpice User's Guide
Index
worst-case timing analysis, digital, 594–608
Y
y-axis
adding a second y-axis, 671
Z
zoom regions, Probe windows, 674
805
Index
806
Product Version 10.5
PSpice User's Guide