HSPICE Reference Manual: Commands and Control Options

HSPICE Reference Manual: Commands and Control Options
HSPICE® Reference
Manual: Commands and
Control Options
Version E-2010.12, December 2010
Copyright Notice and Proprietary Information
Copyright © 2010 Synopsys, Inc. All rights reserved. This software and documentation contain confidential and proprietary
information that is the property of Synopsys, Inc. The software and documentation are furnished under a license agreement and
may be used or copied only in accordance with the terms of the license agreement. No part of the software and documentation may
be reproduced, transmitted, or translated, in any form or by any means, electronic, mechanical, manual, optical, or otherwise, without
prior written permission of Synopsys, Inc., or as expressly provided by the license agreement.
Right to Copy Documentation
The license agreement with Synopsys permits licensee to make copies of the documentation for its internal use only.
Each copy shall include all copyrights, trademarks, service marks, and proprietary rights notices, if any. Licensee must
assign sequential numbers to all copies. These copies shall contain the following legend on the cover page:
“This document is duplicated with the permission of Synopsys, Inc., for the exclusive use of
__________________________________________ and its employees. This is copy number __________.”
Destination Control Statement
All technical data contained in this publication is subject to the export control laws of the United States of America.
Disclosure to nationals of other countries contrary to United States law is prohibited. It is the reader’s responsibility to
determine the applicable regulations and to comply with them.
Disclaimer
SYNOPSYS, INC., AND ITS LICENSORS MAKE NO WARRANTY OF ANY KIND, EXPRESS OR IMPLIED, WITH
REGARD TO THIS MATERIAL, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF
MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE.
Registered Trademarks (®)
Synopsys, AMPS, Astro, Behavior Extracting Synthesis Technology, Cadabra, CATS, Certify, CHIPit, CoMET, Design
Compiler, DesignWare, Formality, Galaxy Custom Designer, HAPS, HapsTrak, HDL Analyst, HSIM, HSPICE, Identify,
Leda, MAST, METeor, ModelTools, NanoSim, OpenVera, PathMill, Physical Compiler, PrimeTime, SCOPE, Simply Better
Results, SiVL, SNUG, SolvNet, Syndicated, Synplicity, the Synplicity logo, Synplify, Synplify Pro, Synthesis Constraints
Optimization Environment, TetraMAX, UMRBus, VCS, Vera, and YIELDirector are registered trademarks of Synopsys,
Inc.
Trademarks (™)
AFGen, Apollo, Astro-Rail, Astro-Xtalk, Aurora, AvanWaves, BEST, Columbia, Columbia-CE, Confirma, Cosmos,
CosmosLE, CosmosScope, CRITIC, CustomExplorer, CustomSim, DC Expert, DC Professional, DC Ultra, Design
Analyzer, Design Vision, DesignerHDL, DesignPower, DFTMAX, Direct Silicon Access, Discovery, Eclypse, Encore,
EPIC, Galaxy, HANEX, HDL Compiler, Hercules, Hierarchical Optimization Technology, High-performance ASIC
Prototyping System, HSIMplus, i-Virtual Stepper, IICE, in-Sync, iN-Tandem, Jupiter, Jupiter-DP, JupiterXT,
JupiterXT-ASIC, Liberty, Libra-Passport, Library Compiler, Magellan, Mars, Mars-Rail, Mars-Xtalk, Milkyway,
ModelSource, Module Compiler, MultiPoint, Physical Analyst, Planet, Planet-PL, Polaris, Power Compiler, Raphael,
Saturn, Scirocco, Scirocco-i, Star-RCXT, Star-SimXT, StarRC, System Compiler, System Designer, Taurus, TotalRecall,
TSUPREM-4, VCS Express, VCSi, VHDL Compiler, VirSim, and VMC are trademarks of Synopsys, Inc.
Service Marks (sm)
MAP-in, SVP Café, and TAP-in are service marks of Synopsys, Inc.
SystemC is a trademark of the Open SystemC Initiative and is used under license.
ARM and AMBA are registered trademarks of ARM Limited.
Saber is a registered trademark of SabreMark Limited Partnership and is used under license.
All other product or company names may be trademarks of their respective owners.
ii
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Contents
1.
2.
HSPICE and HSPICE RF Application Commands. . . . . . . . . . . . . . . . . . . .
1
hspice. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2
Examples of Starting HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9
Using HSPICE for Calculating New Measurements. . . . . . . . . . . . . . . . .
10
hspicerf . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
12
HSPICE and HSPICE RF Netlist Commands . . . . . . . . . . . . . . . . . . . . . . . .
13
HSPICE and RF Commands Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14
Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14
Alter Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
Conditional Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
Digital Vector . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
Encryption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
Field Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
Input/Output Buffer Information Specification (IBIS) . . . . . . . . . . . . . . . .
17
Library Management . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
Model and Variation Definition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
Node Naming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
Output Porting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
Simulation Runs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
Verilog-A. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
Alphabetical Listing of Commands. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
.AC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
25
.ACMATCH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
28
.ACPHASENOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
30
.ALIAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
31
.ALTER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
33
.APPENDMODEL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
35
.BA_ACHECK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
36
iii
Contents
.BIASCHK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
iv
38
.CFL_PROTOTYPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
44
.CHECK EDGE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
48
.CHECK FALL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
50
.CHECK GLOBAL_LEVEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
51
.CHECK HOLD. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
52
.CHECK IRDROP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
54
.CHECK RISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
56
.CHECK SETUP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
58
.CHECK SLEW . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
59
.CONNECT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
61
.DATA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
64
.DC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
71
.DCMATCH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
76
.DCSENS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
78
.DCVOLT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
80
.DEL LIB. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
81
.DESIGN_EXPLORATION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
84
.DISTO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
86
.DOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
88
.EBD. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
90
.ELSE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
92
.ELSEIF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
93
.END. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
94
.ENDDATA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
95
.ENDIF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
96
.ENDL (or) .ENDL TT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
97
.ENDS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
98
.ENV. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
99
.ENVFFT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
100
.ENVOSC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
101
.EOM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
102
.FFT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
103
.FLAT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
108
.FOUR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
110
.FSOPTIONS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
111
.GLOBAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
114
.HB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
115
.HBAC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
118
Contents
.HBLIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
119
.HBLSP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
121
.HBNOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
123
.HBOSC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
126
.HBXF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
131
.HDL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
132
.IBIS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
134
.IC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
138
.ICM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
140
.IF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
142
.INCLUDE (or) .INC (or) .INCL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
144
.IVTH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
145
.JITTER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
147
.LAYERSTACK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
148
.LIB. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
150
.LIN. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
154
.LOAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
158
.LPRINT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
160
.LSTB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
161
.MACRO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
164
.MALIAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
167
.MATERIAL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
169
.MEASURE (or) .MEAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
171
.MEASURE (Rise, Fall, Delay, and Power Measurements) . . . . . . . . . . .
173
.MEASURE (FIND and WHEN) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
178
.MEASURE (Continuous Results) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
182
.MEASURE (Equation Evaluation/Arithmetic Expression) . . . . . . . . . . . .
185
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS). . . . . . .
187
.MEASURE (Integral Function) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
191
.MEASURE (Derivative Function) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
193
.MEASURE (Error Function) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
196
.MEASURE PHASENOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
198
.MEASURE PTDNOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
202
.MEASURE (Pushout Bisection) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
203
.MEASURE (ACMATCH) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
205
.MEASURE (DCMATCH) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
206
.MEASURE FFT. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
208
.MEASURE LSTB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
211
.MODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
213
v
Contents
.MODEL_INFO. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
vi
221
.MOSRA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
222
.MOSRAPRINT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
226
.MOSRA_SUBCKT_PIN_VOLT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
227
.NODESET. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
228
.NOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
230
.OP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
233
.OPTION (or) .OPTIONS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
235
.PARAM (or) .PARAMETER (or) .PARAMETERS . . . . . . . . . . . . . . . . . .
237
.PAT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
241
.PHASENOISE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
244
.PKG. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
247
.POWER. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
249
.POWERDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
251
.PRINT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
252
.PROBE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
255
.PROTECT or .PROT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
258
.PTDNOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
259
.PZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
263
.SAMPLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
265
.SAVE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
266
.SENS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
268
.SHAPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
270
.SHAPE (Defining Rectangles) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
271
.SHAPE (Defining Circles) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
272
.SHAPE (Defining Polygons) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
273
.SHAPE (Defining Strip Polygons) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
275
.SHAPE (Defining Trapezoids) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
276
.SN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
277
.SNAC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
279
.SNFT. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
280
.SNNOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
283
.SNOSC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
285
.SNXF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
288
.STATEYE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
290
.STIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
294
.STORE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
298
.SUBCKT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
301
.SURGE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
306
Contents
3.
.SWEEPBLOCK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
307
.TEMP (or) .TEMPERATURE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
309
.TF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
312
.TITLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
313
.TRAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
314
.TRANNOISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
320
.UNPROTECT or .UNPROT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
324
.VARIATION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
325
.VEC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
327
HSPICE and RF Netlist Simulation Control Options. . . . . . . . . . . . . . . . . .
329
HSPICE Control Options Grouped By Function. . . . . . . . . . . . . . . . . . . . . . . .
330
General Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
330
Input/Output Controls . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
331
Model Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
332
HSPICE Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
334
Transient and AC Small Signal Analysis Options . . . . . . . . . . . . . . . . . . .
334
HSPICE RF Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
336
HB Options. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
336
Phase Noise Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
336
Power Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
337
RC Network Reduction. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
337
Simulation Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
337
Shooting Newton Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
337
DSPF Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
338
SPEF Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
338
Transient Accuracy Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
338
Alphabetical Listing of HSPICE Control Options . . . . . . . . . . . . . . . . . . . . . . .
339
.OPTION ABSH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
352
.OPTION ABSI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
353
.OPTION ABSIN. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
354
.OPTION ABSMOS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
355
.OPTION ABSTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
356
.OPTION ABSV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
357
.OPTION ABSVAR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
358
.OPTION ABSVDC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
359
.OPTION ACCURATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
360
.OPTION ACOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
361
vii
Contents
.OPTION ALTCC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
viii
362
.OPTION ALTCHK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
363
.OPTION APPENDALL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
364
.OPTION ARTIST. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
366
.OPTION ASPEC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
367
.OPTION AUTOSTOP (or) .OPTION AUTOST . . . . . . . . . . . . . . . . . . . .
368
.OPTION BA_ACTIVE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
370
.OPTION BA_ACTIVEHIER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
371
.OPTION BA_ADDPARAM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
372
.OPTION BA_COUPLING . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
373
.OPTION BA_DPFPFX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
374
.OPTION BA_ERROR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
375
.OPTION BA_FILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
376
.........................................................
.OPTION BA_FINGERDELIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
377
.OPTION BA_GEOSHRINK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
378
.........................................................
.OPTION BA_HIERDELIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
379
.........................................................
.OPTION BA_IDEALPFX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
380
.OPTION BA_MERGEPORT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
381
.OPTION BA_NETFMT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
382
.OPTION BA_PRINT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
383
.OPTION BA_SCALE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
384
.OPTION BA_TERMINAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
385
.OPTION BADCHR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
387
.OPTION BDFATOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
388
.OPTION BDFRTOL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
390
.OPTION BEEP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
392
.OPTION BIASFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
393
.OPTION BIASINTERVAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
394
.OPTION BIASNODE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
395
.OPTION BIASPARALLEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
396
.OPTION BIAWARN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
397
.OPTION BINPRNT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
398
.OPTION BPNMATCHTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
399
.OPTION BRIEF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
400
.OPTION BSIM4PDS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
401
.OPTION BYPASS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
402
Contents
.OPTION BYTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
403
.OPTION CAPTAB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
404
.OPTION CFLFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
405
.OPTION CHGTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
406
.OPTION CMIMCFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
407
.OPTION CMIFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
408
.OPTION CMIPATH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
409
.OPTION CMIUSRFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
410
.OPTION CONVERGE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
412
.OPTION CPTIME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
413
.OPTION CSCAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
414
.OPTION CSDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
415
.OPTION CSHDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
416
.OPTION CSHUNT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
417
.OPTION CUSTCMI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
418
.OPTION CVTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
419
.OPTION D_IBIS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
420
.OPTION DCAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
421
.OPTION DCCAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
422
.OPTION DCFOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
423
.OPTION DCHOLD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
424
.OPTION DCIC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
425
.OPTION DCON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
426
.OPTION DCSTEP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
427
.OPTION DCTRAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
428
.OPTION DEFAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
429
.OPTION DEFAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
430
.OPTION DEFL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
431
.OPTION DEFNRD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
432
.OPTION DEFNRS. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
433
.OPTION DEFPD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
434
.OPTION DEFPS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
435
.OPTION DEFSA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
436
.OPTION DEFSB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
437
.OPTION DEFSD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
438
.OPTION DEFW. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
439
.OPTION DEGF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
440
.OPTION DEGFN. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
441
.OPTION DEGFP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
442
ix
Contents
.OPTION DELMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
x
443
.OPTION DI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
444
.OPTION DIAGNOSTIC (or) .OPTION DIAGNO . . . . . . . . . . . . . . . . . . .
445
.OPTION DLENCSDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
446
.OPTION DV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
447
.OPTION DVDT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
448
.OPTION DVTR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
449
.OPTION DYNACC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
450
.OPTION EM_RECOVERY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
451
.OPTION EPSMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
452
.OPTION EXPLI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
453
.OPTION EXPMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
454
.OPTION FAST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
455
.OPTION FFT_ACCURATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
456
.OPTION FFTOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
457
.OPTION FMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
458
.OPTION FS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
459
.OPTION FSCAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
460
.OPTION FT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
461
.OPTION GDCPATH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
462
.OPTION GENK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
463
.OPTION GEOSHRINK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
464
.OPTION GMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
465
.OPTION GMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
466
.OPTION GMINDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
467
.OPTION GRAMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
468
.OPTION GSCAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
469
.OPTION GSHDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
470
.OPTION GSHUNT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
471
.OPTION HBACKRYLOVDIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
472
.OPTION HBACKRYLOVITER (or) HBAC_KRYLOV_ITER . . . . . . . . . . .
473
.OPTION HBACTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
474
.OPTION HBCONTINUE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
475
.OPTION HBFREQABSTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
476
.OPTION HBFREQRELTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
477
.OPTION HB_GIBBS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
478
.OPTION HBJREUSE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
479
.OPTION HBJREUSETOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
480
.OPTION HBKRYLOVDIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
481
Contents
.OPTION HBKRYLOVTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
482
.OPTION HBKRYLOVMAXITER (or) HB_KRYLOV_MAXITER . . . . . . . .
483
.OPTION HBLINESEARCHFAC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
484
.OPTION HBMAXITER (or) HB_MAXITER . . . . . . . . . . . . . . . . . . . . . . .
485
.OPTION HBOSCMAXITER (or) HBOSC_MAXITER . . . . . . . . . . . . . . .
486
.OPTION HBPROBETOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
487
.OPTION HBSOLVER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
488
.OPTION HBTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
489
.OPTION HBTRANFREQSEARCH . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
490
.OPTION HBTRANINIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
491
.OPTION HBTRANPTS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
492
.OPTION HBTRANSTEP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
493
.OPTION HIER_DELIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
494
.OPTION HIER_SCALE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
495
.OPTION IC_ACCURATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
497
.OPTION ICSWEEP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
498
.OPTION IMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
499
.OPTION IMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
500
.OPTION INGOLD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
501
.OPTION INTERP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
503
.OPTION IPROP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
504
.OPTION ITL1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
505
.OPTION ITL2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
506
.OPTION ITL3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
507
.OPTION ITL4 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
508
.OPTION ITL5 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
509
.OPTION ITLPTRAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
510
.OPTION ITLPZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
511
.OPTION ITRPRT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
512
.OPTION IVTH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
513
.OPTION KCLTEST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
514
.OPTION KLIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
515
.OPTION LA_FREQ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
516
.OPTION LA_MAXR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
517
.OPTION LA_MINC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
518
.OPTION LA_TIME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
519
.OPTION LA_TOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
520
.OPTION LENNAM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
521
.OPTION LIMPTS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
522
xi
Contents
.OPTION LIMTIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xii
523
.OPTION LISLVL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
524
.OPTION LIS_NEW . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
525
.OPTION LIST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
526
.OPTION LOADHB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
527
.OPTION LOADSNINIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
528
.OPTION LSCAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
529
.OPTION LVLTIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
531
.OPTION MACMOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
532
.OPTION MAXAMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
534
.OPTION MAXORD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
535
.OPTION MAXWARNS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
536
.OPTION MBYPASS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
537
.OPTION MCBRIEF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
538
.OPTION MEASDGT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
539
.OPTION MEASFAIL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
540
.OPTION MEASFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
541
.OPTION MEASFORM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
542
.OPTION MEASOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
544
.OPTION MESSAGE_LIMIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
545
.OPTION METHOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
546
.OPTION MODMONTE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
549
.OPTION MODPRT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
551
.OPTION MONTECON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
553
.OPTION MOSRALIFE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
554
.OPTION MOSRASORT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
555
.OPTION MRAAPI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
556
.OPTION MRAEXT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
557
.OPTION MRAPAGED . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
558
.OPTION MRA00PATH, MRA01PATH, MRA02PATH, MRA03PATH . . . .
559
.OPTION MTTHRESH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
560
.OPTION MU . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
561
.OPTION NCFILTER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
562
.OPTION NCWARN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
563
.OPTION NEWTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
564
.OPTION NODE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
565
.OPTION NOELCK. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
566
.OPTION NOISEMINFREQ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
567
.OPTION NOMOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
568
Contents
.OPTION NOPIV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
569
.OPTION NOTOP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
570
.OPTION NOWARN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
571
.OPTION NUMDGT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
572
.OPTION NUMERICAL_DERIVATIVES . . . . . . . . . . . . . . . . . . . . . . . . . .
573
.OPTION NXX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
574
.OPTION OFF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
575
.OPTION OPFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
576
.OPTION OPTCON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
577
.OPTION OPTLST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
579
.OPTION OPTPARHIER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
580
.OPTION OPTS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
581
.OPTION PARHIER (or) .OPTION PARHIE . . . . . . . . . . . . . . . . . . . . . .
582
.OPTION PATHNUM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
583
.OPTION PCB_SCALE_FORMAT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
584
.OPTION PHASENOISEKRYLOVDIM . . . . . . . . . . . . . . . . . . . . . . . . . .
586
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER 587
.OPTION PHASENOISETOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
588
.OPTION PHASETOLI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
589
.OPTION PHASETOLV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
590
.OPTION PHD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
591
.OPTION PHNOISELORENTZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
592
.OPTION PHNOISEAMPM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
593
.OPTION PIVOT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
594
.OPTION PIVTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
595
.OPTION POST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
596
.OPTION POSTLVL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
598
.OPTION POST_VERSION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
599
.OPTION POSTTOP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
601
.OPTION PROBE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
602
.OPTION PSF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
603
.OPTION PURETP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
604
.OPTION PUTMEAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
605
.OPTION PZABS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
606
.OPTION PZTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
607
.OPTION RADEGFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
608
.OPTION RADEGOUTPUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
609
.OPTION RANDGEN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
610
.OPTION REDEFSUB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
611
xiii
Contents
.OPTION RELH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xiv
612
.OPTION RELI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
613
.OPTION RELIN. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
614
.OPTION RELMOS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
615
.OPTION RELQ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
616
.OPTION RELTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
617
.OPTION RELV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
618
.OPTION RELVAR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
619
.OPTION RELVDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
620
.OPTION REPLICATES . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
621
.OPTION RES_BITS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
622
.OPTION RESMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
623
.OPTION RISETIME (or) .OPTION RISETI . . . . . . . . . . . . . . . . . . . . . . .
624
.OPTION RITOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
626
.OPTION RMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
627
.OPTION RMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
628
.OPTION RUNLVL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
629
.OPTION SAMPLING_METHOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
633
.OPTION SAVEHB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
635
.OPTION SAVESNINIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
636
.OPTION SCALE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
637
.OPTION SCALM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
638
.OPTION SEARCH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
639
.OPTION SEED . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
640
.OPTION SHRINK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
641
.OPTION SIM_ACCURACY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
642
.OPTION SIM_DELTAI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
643
.OPTION SIM_DELTAV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
644
.OPTION SIM_DSPF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
645
.OPTION SIM_DSPF_ACTIVE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
647
.OPTION SIM_DSPF_INSERROR . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
648
.OPTION SIM_DSPF_LUMPCAPS . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
649
.OPTION SIM_DSPF_MAX_ITER . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
650
.OPTION SIM_DSPF_RAIL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
651
.OPTION SIM_DSPF_SCALEC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
652
.OPTION SIM_DSPF_SCALER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
653
.OPTION SIM_DSPF_VTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
654
.OPTION SIM_LA. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
656
.OPTION SIM_LA_FREQ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
657
Contents
.OPTION SIM_LA_MAXR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
658
.OPTION SIM_LA_MINC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
659
.OPTION SIM_LA_TIME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
660
.OPTION SIM_LA_TOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
661
.OPTION SIM_ORDER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
662
.OPTION SIM_OSC_DETECT_TOL . . . . . . . . . . . . . . . . . . . . . . . . . . . .
663
.OPTION SIM_POSTAT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
664
.OPTION SIM_POSTDOWN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
665
.OPTION SIM_POSTSCOPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
666
.OPTION SIM_POSTSKIP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
667
.OPTION SIM_POSTTOP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
668
.OPTION SIM_POWER_ANALYSIS . . . . . . . . . . . . . . . . . . . . . . . . . . . .
669
.OPTION SIM_POWER_TOP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
670
.OPTION SIM_POWERDC_ACCURACY . . . . . . . . . . . . . . . . . . . . . . . .
671
.OPTION SIM_POWERDC_HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . .
672
.OPTION SIM_POWERPOST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
673
.OPTION SIM_POWERSTART . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
674
.OPTION SIM_POWERSTOP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
675
.OPTION SIM_SPEF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
676
.OPTION SIM_SPEF_ACTIVE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
677
.OPTION SIM_SPEF_INSERROR . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
678
.OPTION SIM_SPEF_LUMPCAPS . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
679
.OPTION SIM_SPEF_MAX_ITER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
680
.OPTION SIM_SPEF_PARVALUE . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
681
.OPTION SIM_SPEF_RAIL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
682
.OPTION SIM_SPEF_SCALEC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
683
.OPTION SIM_SPEF_SCALER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
684
.OPTION SIM_SPEF_VTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
685
.OPTION SIM_TG_THETA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
686
.OPTION SIM_TRAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
687
.OPTION SI_SCALE_SYMBOLS. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
688
.OPTION SLOPETOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
689
.OPTION SNACCURACY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
690
.OPTION SNCONTINUE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
691
.OPTION SNMAXITER (or) SN_MAXITER . . . . . . . . . . . . . . . . . . . . . . .
692
.OPTION SOIQ0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
693
.OPTION SPLIT_DP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
694
.OPTION SPMODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
696
.OPTION STATFL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
697
xv
Contents
.OPTION STRICT_CHECK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.
xvi
698
.OPTION SX_FACTOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
699
.OPTION SYMB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
700
.OPTION TIMERES . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
701
.OPTION TMIFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
702
.OPTION TMIPATH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
703
.OPTION TMIVERSION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
704
.OPTION TNOM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
705
.OPTION TRANFORHB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
706
.OPTION TRCON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
707
.OPTION TRTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
708
.OPTION UNWRAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
709
.OPTION VAMODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
710
.OPTION VERIFY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
711
.OPTION VFLOOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
712
.OPTION VNTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
713
.OPTION WACC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
714
.OPTION WARN. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
715
.OPTION WARN_SEP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
716
.OPTION WARNLIMIT (or) .OPTION WARNLIM . . . . . . . . . . . . . . . . . .
717
.OPTION WAVE_POP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
718
.OPTION WDELAYOPT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
719
.OPTION WDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
720
.OPTION WINCLUDEGDIMAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
722
.OPTION WL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
723
.OPTION WNFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
724
.OPTION XDTEMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
725
.OPTION (X0R,X0I) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
727
.OPTION (X1R,X1I) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
728
.OPTION (X2R,X21). . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
729
.VARIATION Block Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
730
.DESIGN_EXPLORATION Block Control Options . . . . . . . . . . . . . . . . . .
732
Digital Vector File Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
735
ENABLE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
736
IDELAY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
737
IO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
739
Contents
A.
ODELAY. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
740
OUT or OUTZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
742
PERIOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
743
RADIX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
744
SLOPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
745
TDELAY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
747
TFALL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
749
TRISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
751
TRIZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
753
TSKIP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
754
TUNIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
755
VIH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
757
VIL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
758
VNAME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
759
VOH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
761
VOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
763
VREF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
765
VTH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
766
Obsolete Commands and Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
769
.ACDCFACTOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
770
.GRAPH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
771
.MODEL Command for .GRAPH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
773
.NET. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
775
.PLOT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
777
.WIDTH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
779
.OPTION ACCT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
780
.OPTION ALT999 or ALT9999 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
781
.OPTION BKPSIZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
782
.OPTION CDS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
783
.OPTION CO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
784
xvii
Contents
B.
xviii
.DEGINFO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
785
.OPTION H9007. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
786
.OPTION MEASSORT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
787
.OPTION MENTOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
788
.OPTION MODSRH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
789
.OPTION PIVREF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
791
.OPTION NOPAGE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
792
.OPTION PIVREL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
793
.OPTION PLIM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
794
.OPTION SDA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
795
.OPTION SPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
796
.OPTION SIM_LA_MINMODE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
797
.OPTION ZUKEN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
798
How Options Affect other Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
799
GEAR Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
800
ACCURATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
800
FAST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
800
GEAR Method, ACCURATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
801
ACCURATE, GEAR Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
802
ACCURATE, FAST. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
802
GEAR Method, FAST. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
803
GEAR Method, ACCURATE, FAST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
804
RUNLVL=N. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
804
RUNLVL, ACCURATE, FAST, GEAR method . . . . . . . . . . . . . . . . . . . . . . . . .
805
DVDT=1,2,3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
805
LVLTIM=0,2,3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
805
KCLTEST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
806
BRIEF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
806
Option Notes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
806
RUNLVL Option Notes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
807
Contents
Finding the Golden Reference for Options. . . . . . . . . . . . . . . . . . . . . . . . . . . .
808
Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
809
xix
Contents
xx
About This Manual
This manual describes the individual HSPICE commands you can use to
simulate and analyze your circuit designs.
Inside This Manual
This manual contains the chapters described below. For descriptions of the
other manuals in the HSPICE documentation set, see the next section, The
HSPICE Documentation Set.
Chapter
Description
Chapter 1, HSPICE and
HSPICE RF Application
Commands
Describes the commands you use to start HSPICE
or HSPICE RF, including syntax, arguments, and
examples.
Chapter 2, HSPICE and
HSPICE RF Netlist
Commands
Describes the commands you can use in HSPICE
and HSPICE RF netlists.
Chapter 3, HSPICE and RF
Netlist Simulation Control
Options
Describes the HSPICE and HSPICE RF simulation
control options you can set using various forms of
the .OPTION command.
Chapter 4, Digital Vector File
Commands
Contains an alphabetical listing of the HSPICE
commands you can use in an digital vector file.
Appendix A, Obsolete
Commands and Options
Describes commands and options no longer
commonly used in HSPICE.
Appendix B, How Options
Affect other Options
Describes the effects of specifying control options
on other options in the netlist.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
xxi
The HSPICE Documentation Set
The HSPICE Documentation Set
This manual is a part of the HSPICE documentation set, which includes the
following manuals:
xxii
Manual
Description
HSPICE User Guide:
Simulation and Analysis
Describes how to use HSPICE to simulate and analyze
your circuit designs, and includes simulation
applications. This is the main HSPICE user guide.
HSPICE User Guide:
Signal Integrity
Describes how to use HSPICE to maintain signal
integrity in your chip design.
HSPICE User Guide: RF
Analysis
Describes how to use special set of analysis and design
capabilities added to HSPICE to support RF and highspeed circuit design.
HSPICE Reference
Manual: Elements and
Device Models
Describes standard models you can use when
simulating your circuit designs in HSPICE, including
passive devices, diodes, JFET and MESFET devices,
and BJT devices.
HSPICE Reference
Manual: MOSFET Models
Describes available MOSFET models you can use when
simulating your circuit designs in HSPICE.
HSPICE Integration to
Cadence® Virtuoso®
Analog Design
Environment User Guide
Describes use of the HSPICE simulator integration to
the Cadence tool.
AMS Discovery Simulation
Interface Guide for
HSPICE
Describes use of the Simulation Interface with other
EDA tools for HSPICE.
AvanWaves User Guide
Describes the AvanWaves tool, which you can use to
display waveforms generated during HSPICE circuit
design simulation.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Searching Across the HSPICE Documentation Set
Searching Across the HSPICE Documentation Set
You can access the PDF format documentation from your install directory for
the current release by entering -docs on the terminal command line when the
HSPICE tool is open.
Synopsys includes an index with your HSPICE documentation that lets you
search the entire HSPICE documentation set for a particular topic or keyword.
In a single operation, you can instantly generate a list of hits that are hyperlinked to the occurrences of your search term. For information on how to
perform searches across multiple PDF documents, see the HSPICE release
notes.
Note:
To use this feature, the HSPICE documentation files, the Index
directory, and the index.pdx file must reside in the same
directory. (This is the default installation for Synopsys
documentation.) Also, Adobe Acrobat must be invoked as a
standalone application rather than as a plug-in to your web
browser.
You can also invoke HSPICE and RF documentation in a browser-based help
system by entering-help on your terminal command line when the HSPICE
tool is open. This provides access to all the HSPICE manuals with the
exception of the AvanWaves User Guide which is available in PDF format only.
Known Limitations and Resolved STARs
You can find information about known problems and limitations and resolved
Synopsys Technical Action Requests (STARs) in the HSPICE Release Notes
shipped with this release. For updates, go to SolvNet.
To access the HSPICE Release Notes:
1. Go to https://solvnet.synopsys.com/ReleaseNotes. (If prompted, enter your
user name and password. If you do not have a Synopsys user name and
password, follow the instructions to register with SolvNet.)
2. Select Download Center> HSPICE> version number> Release Notes.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
xxiii
Conventions
Conventions
The following conventions are used in Synopsys HSPICE documentation.
Table 1 Typographical conventions
Convention
Description
Courier
Indicates command syntax.
Italic
Indicates a user-defined value, such as object_name.
Bold
Indicates user input — text you type verbatim —i n syntax and
examples.
Bold indicates a GUI element.
[ ]
Denotes optional parameters, such as:
write_file [-f filename]
...
Indicates that parameters can be repeated as many times as
necessary:
pin1 pin2 ... pinN
|
Indicates a choice among alternatives, such as
low | medium | high
+
Indicates a continuation of a command line.
/
Indicates levels of directory structure.
Edit > Copy
Indicates a path to a menu command, such as opening the
Edit menu and choosing Copy.
Control-c
Indicates a keyboard combination, such as holding down the
Control key and pressing c.
Customer Support
Customer support is available through SolvNet online customer support and
through contacting the Synopsys Technical Support Center.
xxiv
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Customer Support
Accessing SolvNet
SolvNet includes an electronic knowledge base of technical articles and
answers to frequently asked questions about Synopsys tools. SolvNet also
gives you access to a wide range of Synopsys online services, which include
downloading software, viewing Documentation on the Web, and entering a call
to the Support Center.
To access SolvNet:
1. Go to the SolvNet Web page at http://solvnet.synopsys.com.
2. If prompted, enter your user name and password. (If you do not have a
Synopsys user name and password, follow the instructions to register with
SolvNet.)
If you need help using SolvNet, click Help on the SolvNet menu bar.
The link to any recorded training is
https://solvnet.synopsys.com/trainingcenter/view.faces
Access recent release update training by going to
https://solvnet.synopsys.com/search/advanced_search.faces
Contacting the Synopsys Technical Support Center
If you have problems, questions, or suggestions, you can contact the Synopsys
Technical Support Center in the following ways:
■
Open a call to your local support center from the Web by going to
http://solvnet.synopsys.com/EnterACall (Synopsys user name and
password required).
■
Send an e-mail message to your local support center.
■
•
E-mail [email protected] from within North America.
•
Find other local support center e-mail addresses at
http://www.synopsys.com/support/support_ctr.
Telephone your local support center.
•
Call (800) 245-8005 from within the continental United States.
•
Call (650) 584-4200 from Canada.
•
Find other local support center telephone numbers at
http://www.synopsys.com/support/support_ctr.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
xxv
Customer Support
xxvi
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
1
1
HSPICE and HSPICE RF Application Commands
Describes the commands you use to start HSPICE or HSPICE RF, including
syntax, arguments, and examples.
This chapter provides the syntax and arguments for the hspice or hspicerf
application commands. You can enter these commands at the command-line
prompt to start HSPICE or HSPICE RF from the unified HSPICE binary
(hspice) on all primary platforms. (You can run RF features with one HSPICE
license and one HSPICE RF license or with two HSPICE licenses.)
The following sections show you how to invoke:
■
hspice
■
hspicerf
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
1
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
hspice
Invokes HSPICE or HSPICE RF.
Syntax
hspice
[-i path/input_file | -i longpath_exceed256/input_file]
[-o path/output_file | -o longpath_exceed256/output_file]
[-o path [-n number] [-html path/html_file] [-d]
[-C path/input_file] [-CC path/input_file] [-I] [-K]
[-L command_file] [-S] [-case 0|1]
[-dp dp# [-dpconfig dpconfig_file] [-merge]
[-mp process_count] [-mt thread_count] [-hpp]
[-meas measure_file] [-top subcktname]
[-restore checkpoint_file.store.gz]
[-hdl file_name][-hdlpath pathname]
[-vamodel name] [-vamodel name2...]
[-help] [-doc] [-h] [-v]
Argument
Description
-i path/input_file
Input netlist file name for which an extension *.ext is optional. If you
do not specify an input file name extension in the command, HSPICE
searches
■
■
for a *.sp# file, or
for a *.tr#, *.ac#, or *.sw# file (PSF files are not supported).
HSPICE uses the input file name as the root for the output files. To
exceed 256 character use the -i longpath_exceed256/
filename command. HSPICE also checks for an initial conditions
file (.ic) that has the input file root name. The following is an example
of an input file name: /usr/sim/work/rb_design.sp
In this file name:
■
■
■
2
/usr/sim/work/ is the directory path to the design
rb_design is the design root name
.sp is the file name suffix
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-o path/output_file Name of the output file. Here, output_file is the root name of the
output file. HSPICE appends the .lis extension to all output files. For
example:
■
For the output log file: output_file.lis
For transient waveform: output_file.tr0
■
For transient measurement: output_file.mt0
Everything up to the last period is the root file name and everything
after the last period is the file name extension.
■
■
If you either do not use this option or you use it without specifying
a file name, HSPICE uses the output root file name specified in
the -html option. To turn off the html popup, use the -o following
the input file name.
■
If you include the .lis extension in the file name that you enter
using this option, then HSPICE does not append another .lis
extension to the root file name of the output file.
■
If you do not specify an output file name, HSPICE directs output
to stdout.
For the .meas option, some case results differ from the measure
result HSPICE produces. To exceed 256 character use the -o
longpath_exceed256/filename command.
-n number
Starting number for numbering output data file revisions
(output_file.tr#, output_file.ac#, output_file.sw#,
where # is between 0 and 9999.).
-html path/
html_file
HTML output file.
-d
3
■
If a path is unspecified, HSPICE saves the HTML output file in the
same directory that you specified in the -o option.
■
If you do not specify an -o option, HSPICE saves the HTML
output in the working directory.
■
If you do not specify an output file name in either the
-o or -html option, then HSPICE uses the input root file name
as the output file root file name.
If you add .option itrprt = 1 to your netlist to print output variables at
their internal time points, and you use the
-html option when invoking HSPICE, then HSPICE prints the
values to a separate file (*.printtr0).
(UNIX) Displays the content of .st0 files on screen while running
HSPICE. For example, to show the status during simulation.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-C path/input_file
Client/Server (C/S) mode.
■
Entering hspice -C checks out an HSPICE license and starts
client/server mode.
■
Entering hspice -C path/input_file simulates your netlist.
■
Entering hspice -C -K releases the HSPICE license and exits.
For additional information, see Using HSPICE in Client-Server Mode
in the HSPICE User Guide: Simulation and Analysis.
-CC path/input_file Advanced Client/Server mode.
■
Entering hspice -CC checks out an HSPICE license and starts the
advanced client/server mode.
■
Entering hspice -CC path/input_file simulates your netlist.
■
Adding -mp [process_count] enables multiprocessing in the file
contains .Alter, Tran sweeps, or Monte Carlo trials.
■
Entering hspice -CC -share common.sp -o output redirects share
file to avoid issues with *.lis file for the shared model file while
running the multiple servers on a farm or multi-CPU machine.
■
Entering hspice -CC -K releases the HSPICE license and exits.
For additional information, see Launching the Advanced ClientServer Mode (-CC) in the HSPICE User Guide: Simulation and
Analysis
-I
Interactive mode.
■
Entering hspice -I invokes interactive mode.
Entering help at the HSPICE prompt lists supported commands.
■
Entering hspice -I -L file_name runs a command file.
■
Entering quit at the HSPICE exits interactive mode.
For additional information, see “Using Interactive Mode” in the
HSPICE User Guide: Simulation and Analysis.
■
-K
Used with -C option to terminate client/server mode and exit.
-L file_name
Used with -I option to run commands contained in a command file.
-S
Performs as a server. Accepts data from SPEED2000, simulates the
circuit, and returns results to SPEED2000.
■
■
4
On UNIX and Linux, HSPICE waits for successive simulations
after invocation.
On Windows you must re-invoke for each successive simulation.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-case 0|1
■
0: (default) case sensitivity disabled
1: case sensitivity enabled
Enables case sensitivity only for the following items (HSPICE
commands and control options continue to be case-insensitive):
■
■
■
■
■
■
■
■
■
■
Parameter Names
Node Names
Instance Names
Model Names
Subcircuit Names
Data Names
Measure Names
File Names and Paths (case sensitive by default)
Library Entry Names
■
-dp dp#
[-dpconfig
dpconfig_file]
[-merge]
Invokes distributed processing and specifies number of
processes.
■
Specifies the configuration file for DP. HSPICE runs DP on a single
local machine if this option is not specified.
■
Merges the output files from HSPICE. DP only merges the output
files if this option is specified.
For details see Running Distributed Processing (DP) on a Network
Grid in the HSPICE User Guide: Simulation and Analysis.
-hpp
Enables HSPICE Performance Precision. The multicore algorithm
can be applied without multithreading (-mt), but for best
performance, use -hpp -mt N, together, where N is number of
threads. For details, see the HSPICE User Guide: Simulation and
Analysis, Chapter 3, Setup and Simulation, section HSPICE
Precision Parallel (-hpp).
-mp [process_count] Activates multiprocessing while running ALTER cases, transient
sweeps, and Monte Carlo analyses on one machine with multiple
processors/cores. If you specify the number of CPUs you can limit the
number of CPUs to avoid overtaxing performance scalability. If a
CPU number is not specified, HSPICE auto-determines the child
processes by the number of available CPUs. For details see
Multiprocessing (MP) DC Monte Carlo in the HSPICE User Guide:
Simulation and Analysis.
5
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-mt thread_count
Invokes multithreading and specifies the number of processors for a
multithreaded simulation. If thread_count is not entered, HSPICE
issues an error.
For additional information, see Running Multithread/Multiprocess
HSPICE Simulations in the HSPICE User Guide: Simulation and
Analysis. See also .OPTION MTTHRESH in this manual.
-hpp
Enables HSPICE Performance Precision. The multicore algorithm
can be applied without multithreading (-mt), but for best
performance, use -hpp -mt N, together, where N is number of
threads. For details, see the HSPICE User Guide: Simulation and
Analysis, Chapter 3 , Setup and Simulation, section HSPICE
Precision Parallel (-hpp).
-meas measure_file
Re-invokes the measure file to calculate new measurements from a
previous simulation. The format of measure_file is similar to the
HSPICE netlist format. The first line is a comment line and the last
line is an .END command. The following netlist commands are
supported.
■
.MEASURE
.PARAM
■
.TEMP
■
.OPTION
■
.DATA
■
.ENDDATA
■
.FFT
■
.MEASURE FFT
■
.END
Note: The .DATA command in the measure file must be consistent
with the .DATA command in the wavefile.
■
The following types of .OPTION commands are supported:
■
MEASFAIL
NUMDGT
■
INGOLD
■
MEASDGT
■
EM_RECOVERY
Warnings are issued if other options or commands are used. Wave
files formatted as PSF, CSDF, and WDF are not supported.
Syntax to perform spectrum analysis measurements from previous
simulation results:
hspice -i *.tr0 -meas measure_file
■
6
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-top subcktname
Top level subcircuit name. Effectively eliminates the need for defining
“.subckt subcktname“and corresponding “.ends“statements.
Users do not need to instantiate top-level SUBCKT using “X” syntax
of HSPICE.
-restore
checkpoint_file.
store.gz
The checkpoint_file specifies from which simulation the
checkpoint data is to be restored.
The restore operation should be submitted on a machine that has the
same kernel version as the machine used to store, otherwise, a
failure may occur.
Note: Do not use -o outputfile to specify output files; the output
files will be the same as were used in the previous simulation.
Any output files generated by the previous simulation should not be
removed. After the restore simulation is done, the output files will be
updated. For example:
hspice -restore test_1000.store.gz.
The simulation starts from the time point that data was stored at in
the previously interrupted simulation. The data files are named
test_1000.store.gz, and test_1000.tar.
See Storing and Restoring Checkpoint Files (HSPICE) for full details.
-hdl file_name
Verilog-A module. The Verilog-A file is assumed to have a *.va
extension when only a prefix is provided. One -hdl option can include
one Verilog-A file, use multiple -hdl options if multiple Verilog-A files
are needed. This example loads the amp.va Verilog-A source file:
hspice amp.sp -hdl amp.va
When a module to be loaded has the same name as a previouslyloaded module or the names differ in case only, the latter one is
ignored and the simulator issues a warning message.
If a Verilog-A module file is not found or the Compiled Model Library
file has an incompatible version, the simulation exits and an error
message is issued.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
7
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-hdlpath pathname
Search path for a Verilog-A file if HSPICE cannot find it in the current
working directory. The search order for Verilog-A files is:
1. Current working directory
2. Path defined by command-line argument -hdlpath
3. Path defined by environment variable HSP_HDL_PATH
The path defined by either -hdlpath or HSP_HDL_PATH can consist
a set of directory names. The path separator must follow HSPICE
conventions or platform conventions (“;” on UNIX). Path entries that
do not exist are ignored and no error/warning messages are issued.
This example first searches the current working directory and when
a *.va file is not found, the relative location ./my_modules directory is
searched: hspice amp.sp -hdlpath ./my_modules
-vamodel name
-vamodel name2...
Cell names for Verilog-A definitions. name is the cell name that uses
a Verilog-A definition rather than a subcircuit definition when both
exist. Each -vamodel option can take no more than one name.
Repeat this option if multiple Verilog-A modules are defined. If no
name is supplied after -vamodel, then the Verilog-A definition will be
used whenever it is available.
-help
Searchable browser-based help system for HSPICE/HSPICFE RF.
An html browser must be installed on your machine to access this
help system.
-doc
PDF documentation set user manuals for HSPICE and RF flow.
Requires Adobe Acrobat Reader to be installed on your system. You
can do full text searches of the documentation set. See the Release
Notes for instructions.
-h
Displays a help message and exits.
-v
Outputs version information and exits.
8
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Examples of Starting HSPICE
The following are more examples of commands to start running HSPICE.
■
hspice demo.sp -n 7 > demo.out
This command redirects output to a file instead of stdout. demo.sp is the
input netlist file. The .sp extension is optional. The -n 7 starts the output
data file revision numbers at 7; for example: demo.tr7, demo.ac7,
demo.sw7, and so forth. The > redirects the program output listing to file
demo.out.
■
hspice -i demo.sp
demo is the root input file name. Without the -o argument and without
redirection, HSPICE does not generate an output listing file.
■
hspice -i demo.sp -o demo
demo is the output file root name (designated with the -o option). Output
files are named demo.lis, demo.tr0, demo.st0, and demo.ic0.
■
hspice -i rbdir/demo.sp
demo is the input root file name. HSPICE writes the demo.lis, demo.tr0, and
demo.st0 output files into the directory where you executed the HSPICE
command. It also writes the demo.ic0 output file into the same directory as
the input source—that is, rbdir.
■
hspice -i a.b.sp
a.b is the root name. The output files are ./a.b.lis, ./a.b.tr0, ./a.b.st0, and ./
a.b.ic0.
■
hspice -i a.b -o d.e
a.b is the root name for the input file. d.e is the root output file name,
except for the .ic file to which HSPICE assigns the a.b input file root name.
The output files are d.e.lis, d.e.tr0, d.e.st0, and a.b.ic0.
■
hspice -i a.b.sp -o outdir/d.e
HSPICE writes the output files as: outdir/d.e.lis, outdir/d.e.tr0, outdir/d.e.st0,
and outdir/d.e.ic0.
■
hspice -i indir/a.b.sp -o outdir/d.e.lis
a.b is the root for the .ic file. HSPICE writes the .ic0 file into a file named
indir/a.b.ic0. d.e is the root for the output files.
■
hspice test.sp -o test.lis -html test.html
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
9
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
This command creates output file in both .lis and .html format after
simulating the test.sp input netlist.
■
hspice test.sp -html test.html
This command creates only a .html output file after simulating the test.sp
input netlist.
■
hspice test.sp -o test.lis
This command creates only a .lis output file after simulating the test.sp input
netlist.
■
hspice -i test.sp -o -html outdir/a.html
This command creates output files in both .lis and .html format. Both files
are in the outdir directory and their root file name is a.
■
hspice -i test.sp -o out1/a.lis -html out2/b.html
This command creates output files in both .lis and .html format. The .lis file
is in the out1 directory and its root file name is a. The .html file is in the out2
directory and its root file name is b.
■
hspice -i test.sp -o test -x
This command launches a full parasitic back-annotation for the file named
test.sp.
Using HSPICE for Calculating New Measurements
When you want to calculate new measurements from previous simulation
results produced by HSPICE you can use the following mode to rerun HSPICE
without having to do another simulation:
hspice -meas measurefile -i wavefile -o outputfile
See the following table for arguments and descriptions.
10
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 1: HSPICE and HSPICE RF Application Commands
hspice
Argument
Description
-meas measurefile This format is similar to the HSPICE netlist format. The first line
is a comment line and the last line is an .END command. Seven
commands are supported:
■
.MEASURE
.PARAM
■
.TEMP
■
.OPTION
■
.DATA
■
.ENDDATA
■
.END
Note: The .DATA command in the measure file must be
consistent with the .DATA command in the wavefile.
■
The .OPTION command support four types:
■
MEASFAIL
NUMDGT
■
INGOLD
■
MEASDGT
Warnings are issued if other options or commands are used.
Wave files formatted as PSF and CSDF are not supported.
■
-i wavefile
*.tr#, *.ac#, and *.sw# files produced by HSPICE. Waveform files
formatted as PSF are not supported.
If a plot fails to open, it is due to one of the following reasons:
Waveform file format is not supported.
File format is not understood
File is not found
File larger than max size of x
Note: “x” depends on any file size limitation of your application.
For example, a 2GB file size limitation exists on 32-bit HSPICE
Linux, SuSe versions when reading the waveforms. Solaris has
no such limitation
-o outputfile
Same output files as HSPICE. Some case results are different
from the measure result HSPICE produces due to an accuracy
problem.
-h
Displays a help message and exits.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
11
Chapter 1: HSPICE and HSPICE RF Application Commands
hspicerf
Argument
Description
-v
Outputs version information and exits.
hspicerf
Invokes HSPICE RF in standalone mode. HSPICE RF can be launched with
either the integrated executable (hspice) or in standalone mode (hspicerf).
Syntax
hspicerf [-a] input_file [output_file] [-n] [-h] [-v]
Argument
Description
-a
Generates output to stdout in ASCII format. For example,
% hspicerf -a ckt.in
You can redirect the ASCII output to another file. For example,
% hspicerf -a ckt.in > xt
Output from a .PRINT command goes to an ASCII file with a .print#
or .printac# file extension.
input_file
Name of the input netlist.
output_file
Name of the output listing file.
If specified, the simulation output is written to this file and given
a .lis file extension. For example,
% hspicerf ckt.in xt
automatically sets -a and generates output to xt.lis.
12
-n number
Starting number for numbering output data file revisions
(output_file.tr#, output_file.ac#, output_file.sw#,
where # is between 0 and 9999.).
-h
Returns a help message.
-v
Returns version information.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
2
2
HSPICE and HSPICE RF Netlist Commands
Describes the commands you can use in HSPICE/HSPICE RF netlists.
This chapter provides a list of the HSPICE and HSPICE RF netlist commands,
arranged by task, followed by detailed descriptions of the individual commands.
The netlist commands described in this chapter fall into the following
categories:
■
Alter Block
■
Analysis
■
Conditional Block
■
Digital Vector
■
Encryption
■
Field Solver
■
Files
■
Input/Output Buffer Information Specification (IBIS)
■
Library Management
■
Model and Variation Definition
■
Node Naming
■
Output Porting
■
Setup
■
Simulation Runs
■
Subcircuits
■
Verilog-A
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
13
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Analysis
Use of Example Syntax
To copy and paste proven syntax use the demonstration files shipped with your
installation of HSPICE (see Listing of Demonstration Input Files). Attempting to
copy and paste from the book or help documentation may present unexpected
results, as text used in formatting may include hidden characters, white space,
etc. for visual clarity.
HSPICE and RF Commands Overview
Analysis
Use these commands in your netlist to start different types of HSPICE analysis
to save the simulation results into a file and to load the results of a previous
simulation into a new simulation.
HSPICE
.AC
.DCSENS
.LIN
.PAT
.STATEYE
.ACMATCH
.DISTO
.LSTB
.PZ
.TEMP (or) .TEMPERATURE
.DC
.FFT
.NOISE
.SAMPLE
.TF
.DCMATCH
.FOUR
.OP
.SENS
.TRAN
HSPICE RF Analysis
Use these commands in your RF netlist to run different types of HSPICE RF
analyses, save the simulation results into a file, and to load the results of a
previous simulation into a new simulation.
.AC
.ENVFFT
.LIN
.SN
.ACPHASENOISE
.ENVOSC
.LPRINT
.SNAC
.CHECK EDGE
.FFT
.MEASURE
PHASENOISE
.SNFT
14
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Alter Block
.CHECK FALL
.FOUR
.MEASURE
PTDNOISE
.SNNOISE
.CHECK GLOBAL_LEVEL
.HB
.NOISE
.SNOSC
.CHECK HOLD
.HBAC
.OP
.SNXF
.CHECK IRDROP
.HBLIN
.PHASENOISE
.SURGE
.CHECK RISE
.HBLSP
.POWER
.SWEEPBLOCK
.CHECK SETUP
.HBNOISE
.POWERDC
.TEMP
(or) .TEMPERATURE
.CHECK SLEW
.HBOSC
.PTDNOISE
.TF
.DC
.HBXF
..PZ
.TRAN
.ENV
.
Alter Block
Use these commands in your netlist to run alternative simulations of your netlist
by using different data.
.ALTER
.DEL LIB
.TEMP (or) .TEMPERATURE
Conditional Block
Use these commands in your HSPICE netlist to setup a conditional block.
HSPICE does not execute the commands in the conditional block unless the
specified conditions are true.
.ELSE
.ELSEIF
.ENDIF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
.IF
15
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Digital Vector
Digital Vector
Use these commands in your digital vector (VEC) file.
ENABLE
PERIOD
TRISE
VIL
IDELAY
RADIX
TRIZ
VNAME
IO
SLOPE
TSKIP
VOH
ODELAY
TDELAY
TUNIT
VOL
OUT or OUTZ
TFALL
VIH
VREF
VTH
Encryption
Use these commands in your netlist to mark the start and end of a traditionally
(Freelib) encrypted section of a netlist.
.PROTECT or .PROT
.UNPROTECT or .UNPROT
Field Solver
Use these commands in your netlist to define a field solver.
.FSOPTIONS
.LAYERSTACK
.MATERIAL
.SHAPE
Files
Use this command in your netlist to call other files that are not part of the netlist.
.VEC
16
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Input/Output Buffer Information Specification (IBIS)
Input/Output Buffer Information Specification (IBIS)
Use these commands in your netlist for specifying input/output buffer
information.
.EBD
.IBIS
.ICM
.PKG
Library Management
Use these commands in your netlist to manage libraries of circuit designs and
to call other files when simulating your netlist.
.DEL LIB
.ENDL
(or) .ENDL TT
.INCLUDE
(or) .INC
(or) .INCL
.LIB
.LOAD
Model and Variation Definition
Use these commands in your netlist to define models:
.ALIAS
.APPENDMODEL
.MALIAS
.MODEL
.MOSRA
.MOSRAPRINT
.VARIATION
Node Naming
Use these commands in your netlist to name nodes in circuit designs.
.CONNECT
.GLOBAL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
17
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Output Porting
Output Porting
Use these commands in your netlist to specify the output of a simulation to a
printer or graph. You can also define the parameters to measure and to report
in the simulation output.
.BIASCHK
.MEASURE
(or) .MEAS
.PROBE
.DOUT
.PRINT
.STIM
Setup
Use these commands in your netlist to set up your netlist for simulation.
.DATA
.ENDDATA
.IC
.NODESET
.PARAM
(or) .PARA
METER
(or) .PARA
METERS
.DCVOLT
.GLOBAL
.LOAD
.OPTION
(or) .OPTIONS
.SAVE
.TITLE
Simulation Runs
Use these commands in your netlist to mark the start and end of individual
simulation runs and conditions that apply throughout an individual simulation
run.
.END
.TEMP
(or) .TEMPERATURE
.TITLE
Subcircuits
Use these commands in your netlist to define subcircuits and to add instances
of subcircuits to your netlist.
.ENDS
18
.INCLUDE (or) .INC
(or) .INCL
.MODEL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Verilog-A
.EOM
.MACRO
.SUBCKT
Verilog-A
Use the following command in your netlist to declare the Verilog-A source name
and path within the netlist.
.HDL
Alphabetical Listing of Commands
The following is the alphabetical list of links to the HSPICE/RF command set.
For simulation controls see Chapter 3, HSPICE and RF Netlist Simulation
Control Options.
■
.AC
■
.ACMATCH
■
.ACPHASENOISE
■
.ALIAS
■
.ALTER
■
.APPENDMODEL
■
.BA_ACHECK
■
.BIASCHK
■
.CFL_PROTOTYPE
■
.CHECK EDGE
■
.CHECK FALL
■
.CHECK GLOBAL_LEVEL
■
.CHECK HOLD
■
.CHECK IRDROP
■
.CHECK RISE
■
.CHECK SETUP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
19
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Verilog-A
20
■
.CHECK SLEW
■
.CONNECT
■
.DATA
■
.DC
■
.DCMATCH
■
.DCSENS
■
.DCVOLT
■
.DEL LIB
■
.DESIGN_EXPLORATION
■
.DISTO
■
.DOUT
■
.EBD
■
.ELSE
■
.ELSEIF
■
.END
■
.ENDDATA
■
.ENDIF
■
.ENDL (or) .ENDL TT
■
.ENDS
■
.ENV
■
.ENVFFT
■
.ENVOSC
■
.EOM
■
.FFT
■
.FLAT
■
.FOUR
■
.FSOPTIONS
■
.GLOBAL
■
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Verilog-A
■
.HBAC
■
.HBLIN
■
.HBLSP
■
.HBNOISE
■
.HBOSC
■
.HBXF
■
.HDL
■
.IBIS
■
.IC
■
.ICM
■
.IF
■
.INCLUDE (or) .INC (or) .INCL
■
.IVTH
■
.JITTER
■
.LAYERSTACK
■
.LIB
■
.LIN
■
.LOAD
■
.LPRINT
■
.LSTB
■
.MACRO
■
.MALIAS
■
.MATERIAL
■
.MEASURE (or) .MEAS
■
.MEASURE (Rise, Fall, Delay, and Power Measurements)
■
.MEASURE (FIND and WHEN)
■
.MEASURE (Continuous Results)
■
.MEASURE (Equation Evaluation/Arithmetic Expression)
■
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
21
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Verilog-A
22
■
.MEASURE (Integral Function)
■
.MEASURE (Derivative Function)
■
.MEASURE (Error Function)
■
.MEASURE PHASENOISE
■
.MEASURE PTDNOISE
■
.MEASURE (Pushout Bisection)
■
.MEASURE (ACMATCH)
■
.MEASURE (DCMATCH)
■
.MEASURE FFT
■
.MEASURE LSTB
■
.MODEL
■
.MODEL_INFO
■
.MOSRA
■
.MOSRAPRINT
■
.MOSRA_SUBCKT_PIN_VOLT
■
.NODESET
■
.NOISE
■
.OP
■
.OPTION (or) .OPTIONS
■
.PARAM (or) .PARAMETER (or) .PARAMETERS
■
.PAT
■
.PHASENOISE
■
.PKG
■
.POWER
■
.POWERDC
■
.PRINT
■
.PROBE
■
.PROTECT or .PROT
■
.PTDNOISE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Verilog-A
■
.PZ
■
.SAMPLE
■
.SAVE
■
.SENS
■
.SHAPE
■
.SHAPE (Defining Rectangles)
■
.SHAPE (Defining Circles)
■
.SHAPE (Defining Polygons)
■
.SHAPE (Defining Strip Polygons)
■
.SHAPE (Defining Trapezoids)
■
.SN
■
.SNAC
■
.SNFT
■
.SNNOISE
■
.SNOSC
■
.SNXF
■
.STATEYE
■
.STIM
■
.STORE
■
.SUBCKT
■
.SURGE
■
.SWEEPBLOCK
■
.TEMP (or) .TEMPERATURE
■
.TF
■
.TITLE
■
.TRAN
■
.TRANNOISE
■
.UNPROTECT or .UNPROT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
23
Chapter 2: HSPICE and HSPICE RF Netlist Commands
Verilog-A
24
■
.VARIATION
■
.VEC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.AC
.AC
Performs several types of AC analyses.
Syntax
Single or Double Sweep
.AC type np fstart fstop
.AC type np fstart fstop [SWEEP var [START=]start
+ [STOP=]stop [STEP=]incr]
.AC type np fstart fstop [SWEEP var type np start stop]
.AC type np fstart fstop
+ [SWEEP var START=”param_expr1”
+ STOP=”param_expr2” STEP=”param_expr3”]
.AC type np fstart fstop [SWEEP var start_expr
+ stop_expr step_expr]
Sweep Using Parameters
.AC type np fstart fstop [SWEEP DATA=datanm]
.AC DATA=datanm
.AC DATA=datanm [SWEEP var [START=]start [STOP=]stop
+ [STEP=]incr]
.AC DATA=datanm [SWEEP var type np start stop]
.AC DATA=datanm [SWEEP var START="param_expr"
+ STOP="param_expr2" STEP="param_expr3"]
.AC DATA=datanm [SWEEP var start_expr stop_expr
+ step_expr]
Optimization
.AC DATA=datanm OPTIMIZE=opt_par_fun
+ RESULTS=measnames MODEL=optmod
Monte Carlo
.AC type np fstart fstop [SWEEP MONTE=MCcommand]
Argument
Description
DATA=datanm
Data name, referenced in the .AC command.
incr
Increment value of the voltage, current, element, or model parameter. If you
use type variation, specify the np (number of points) instead of incr.
fstart
Starting frequency. If you use POI (list of points) type variation, use a list of
frequency values, not fstart fstop.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
25
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.AC
Argument
Description
fstop
Final frequency.
MONTE=
MCcommand
Where MCcommand can be any of the following:
■
■
■
■
val Specifies the number of random samples to produce.
val firstrun=num Specifies the sample number on which the simulation
starts.
list num Specifies the sample number to execute.
list(num1:num2 num3 num4:num5) Samples from num1 to num2, sample
num3, and samples from num4 to num5 are executed (parentheses are
optional).
np
Number of points or points per decade or octave, depending on which
keyword precedes it.
start
Starting voltage or current or any parameter value for an element or model.
stop
Final voltage or current or any parameter value for an element or a model.
SWEEP
Second sweep.
TEMP
Temperature sweep
type
Any of the following keywords:
■
■
■
■
DEC – decade variation.
OCT – octave variation.
LIN – linear variation.
POI – list of points.
var
Name of an independent voltage or current source, element or model
parameter or the TEMP (temperature sweep) keyword. HSPICE supports
source value sweep, referring to the source name (SPICE style). If you select
a parameter sweep, a .DATA command and a temperature sweep, then you
must choose a parameter name for the source value. You must also later refer
to it in the .AC command. The parameter name cannot start with V or I.
firstrun
The val value specifies the number of Monte Carlo iterations to perform. The
firstrun value specifies the desired number of iterations. HSPICE runs from
num1 to num1+val-1.
list
Iterations at which HSPICE performs a Monte Carlo analysis. You can write
more than one number after a list. The colon represents “from ... to ...".
Specifying only one number causes to HSPICE run at only the specified point.
26
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.AC
Description
The.AC command is usable in several different formats, depending on the
application as shown in the examples. You can also use the .AC command to
perform data-driven analysis in HSPICE.
If the input file includes an .AC command, HSPICE runs AC analysis for the
circuit over a selected frequency range for each parameter in the second
sweep.
For AC analysis, the data file must include at least one independent AC source
element command (for example, VI INPUT GND AC 1V). HSPICE checks for
this condition and reports a fatal error if you did not specify such AC sources.
Examples
.AC DEC 10 1K 100MEG
This example performs a frequency sweep by 10 points per decade from 1kHz
to 100MHz.
See Also
.DC
.DISTO
.LSTB
.NOISE
.TRAN
Using the .AC Statement
BJT and Diode Examples for the paths to the demo files mextram_ac.sp
and vbic99_ac.sp, which use the .AC command.
Device Optimization Examples for paths to the demo netlists bjtopt.sp and
bjtopt2.sp which use .AC sweep keywords.
MOSFET Device Examples for paths to the demo netlists calcap.sp and
cascode.sp for use of the .AC command.
Applications of General Interest Examples for the paths to the demo files
alm124.sp and quickAC.sp, for.AC command usage.
Transmission (W-element) Line Examples for the paths to the demo files
ex1.sp, ex2.sp, ex3.sp, rlgc.sp, and umodel.sp for .AC command usage.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
27
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ACMATCH
.ACMATCH
Calculates the effects of variations in device characteristics and parasitic
capacitance sensitivities on a circuit's AC response.
Syntax
.ACMATCH OUTVAR [THRESHOLD=T] [FILE=string] [INTERVAL=Int]
+ [Virtual_Sensitivity=Yes|No] [Sens_threshold=x]
+ [Sens_node=(nodei_name,nodej_name),…,
+ (nodem_name,noden_name)]
Argument
Description
OutVar
OutputVariable can be one or several output voltages, difference
voltages, or branch current through an independent voltage source.
The voltage or current specifier is followed by an identifier of the AC
quantity of interest: M: magnitude P: phase R: real part I: imaginary
part
Threshold
Only devices with variation contributions above Threshold are reported
in the table. Results for all devices are displayed if Threshold=0 is set.
The maximum value for Threshold is 1.0, but at least 10 devices (or all)
are displayed. Default is 0.01.
File
Valid file name for the output tables. Default is basename.am#, where
# is the regular HSPICE sequence number.
Interval
This option applies to the frequency sweep definition in he .AC
command. A table is printed at the first sweep point, then for each
subsequent increment of SweepValue, and at the final sweep point.
Virtual_Sensitivity
Invokes ACmatch computation and output of virtual sensitivity;
sensitivity table is printed even if variation block does not exist in netlist.
Default: Yes
Sens_Threshold=x Only nodes with sensitivity above x are reported. At least 10
sensitivities (or all) are displayed. This avoids generation of null output
if you specify too large a value for x. Default: 1e-6
Sens_Node
28
Output all sensitivities associated with the requested nodes. The node
name should appear in pairs. (See examples below.)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ACMATCH
Description
Use to calculate the effects of variations in device characteristics on a circuit's
AC response. ACMatch allows for calculation of parasitic capacitor sensitivities
whose nominal values are “zero” in the original design. Such analysis is useful
for high precision (differential) analog circuits and switched capacitor filters. If
more than one ACMatch analysis is specified per simulation, only the last
command is executed. dB syntax is supported in .ACMatch for Vdb and Idb,
for local, global, and element variation.
Note:
ACMatch does not support Spatial Variations.
Examples
.ACMATCH VM(out) VP(out) IM(x1.r1) IP(x1.r1) IM(c1) IP(c1)
.AC dec 10 1k 10Meg interval=10
When using the virtual capacitance sensitivity option Sens_Node multiple
name pairs are supported with one comma between node names, but commas
are optional between node name pairs. Either of the following specifications is
valid in HSPICE:
.ACmatch v(out) virtual_sens=yes
+ sens_node= (out, xi82.net044),
+ (0,out), (xi82.net044,xi82.net031) sens_threshold=1e-6
OR
.ACmatch v(out) virtual_sens=yes
+ sens_node= (out, xi82.net044)
+ (0,out) (xi82.net044,xi82.net031) sens_threshold=1e-6
See Also
.AC
.MEASURE (or) .MEAS
.MEASURE (ACMATCH)
.OPTION POST
ACMatch Analysis
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
29
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ACPHASENOISE
.ACPHASENOISE
Helps you interpret signal and noise quantities as phase variables for
accumulated jitter for closed-loop PLL analysis.
Syntax
.ACPHASENOISE output input [interval] carrier=freq
+ [listfreq=(frequencies|none|all)]
+ [listcount=val] [listfloor=val]
+ [listsources=(1|0)]
Description
The .ACPHASENOISE command aids in the ability to compute “Accumulated
Jitter” or “Timing Jitter” for the closed loop PLL. The accumulated jitter
response is essentially an integral transformation of the closed-loop PLL
response. The .ACPHASENOISE analysis outputs raw data to *.pn0 and
*.printpn0 files. The PHNOISE data is given in units of dBc/Hz, i.e., dB relative
to the carrier, per Hz, across the output nodes specified by the
.ACPHASENOISE command. The data plot is a function of offset frequency. If
the “JITTER” keyword is present, .ACPHASENOISE also outputs the
accumulated TIE jitter data to *.jt0 and *.printjt0 data files. These data are
plotted as a function of time in units of seconds. The Timing Jitter data itself has
units of seconds. The timing jitter calculations make use of the parameters
given in the .ACPHASENOISE syntax, such as “freq” and “interval”.
For details, see Small-Signal Phase-Domain Noise Analysis
(.ACPHASENOISE) in the HSPICE User Guide: RF Analysis.
30
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ALIAS
.ALIAS
Renames a model or library containing a model; deletes an entire library of
models.
Syntax
.ALIAS model_name1 model_name2
Description
Use in instances when you have used .ALTER commands to rename a model,
to rename a library containing a model, or to delete an entire library of models
in HSPICE. If your netlist references the old model name, then after you use
one of these types of .ALTER commands, HSPICE no longer finds this model.
For example, if you use .DEL LIB in the .ALTER block to delete a library, the
.ALTER command deletes all models in this library. If your netlist references
one or more models in the deleted library, then HSPICE no longer finds the
models.
To resolve this issue, HSPICE provides an .ALIAS command to let you keep
the old model name that HSPICE can find in the existing model libraries.
Examples
Example 1
For a scenario in which you delete a library named poweramp that
contains a model named pa1, while another library contains an
equivalent model named par: You can then convert the pa1 model name
to the par1 model name.
.ALIAS pa1 par1
Example 2
During simulation when HSPICE encounters a model named pa1 in your
netlist, it initially cannot find this model because you used an .ALTER
command to delete the library that contained the model. However,
the .ALIAS command indicates to use the par1 model in place of the old
pa1 model and HSPICE does find this new model in another library
so simulation continues.You must specify an old model name and a
new model name to use in its place. You cannot use .ALIAS without any
model names:
.ALIAS
or with only one model name:
.ALIAS pa1
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
31
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ALIAS
Example 3
You also cannot alias a model name to more than one model name
because the simulator cannot determine which of these new models to
use in place of the deleted or renamed model. For the same reason, you
cannot substitute a model name to a second model name and then
substitute the second model name to a third model name.
.ALIAS pa1 par1 par2
Example 4
If your netlist does not contain an .ALTER command and if the .ALIAS
does not report a usage error, then the .ALIAS does not affect the
simulation results.
.ALIAS pa1 par1
.ALIAS par1 par2
Your netlist might contain the command:
.ALIAS myfet nfet
Without an .ALTER command, HSPICE does not use nfet to replace myfet
during simulation.
If your netlist contains one or more .ALTER commands, the first simulation
uses the original myfet model. After the first simulation if the netlist references
myfet from a deleted library, .ALIAS substitutes nfet in place of the missing
model.
■
If HSPICE finds model definitions for both myfet and nfet, it reports an
error and aborts.
■
If HSPICE finds a model definition for myfet, but not for nfet, it reports a
warning and simulation continues by using the original myfet model.
■
If HSPICE finds a model definition for nfet, but not for myfet, it reports a
“replacement successful” message.
See Also
.ALTER
.MALIAS
32
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ALTER
.ALTER
Reruns an HSPICE/HSPICE RF simulation using different parameters and
data.
Syntax
.ALTER title_string
Argument
Description
title_string
Any string up to 80 characters. HSPICE prints the appropriate title
string for each .ALTER run in each section heading of the output listing
and in the graphical data (.tr#) files.
Description
Use this command to rerun an HSPICE simulation using different parameters
and data. Use parameter (variable) values for .PRINT commands before you
alter them. The .ALTER block cannot include .PRINT, or any other input/
output commands. You can include analysis commands
(.DC, .AC, .TRAN, .FOUR, .DISTO, .PZ, and so on) in a .ALTER block in an
input netlist file.
However, if you change only the analysis type and you do not change the circuit
itself, then the simulation runs faster if you specify all analysis types in one
block, instead of using separate .ALTER blocks for each analysis type.
To activate multiprocessing while running .ALTER cases, enter hspice -mp on
the command line. While running in parallel mode, HSPICE checks if the input
case has .ALTER commands. If it has, HSPICE splits the input case into
several subcases, then fork HSPICE processes to run each subcase at the
same time. After all HSPICE processes finish running the subcases, HSPICE
merges all the output files of the subcases.
The .ALTER sequence or block can contain:
■
Element commands (except E, F, G, H, I, and V source elements)
■
.AC commands
■
.ALIAS commands
■
.DATA commands
■
.DC commands
■
.DEL LIB commands
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
33
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ALTER
■
.HDL commands
■
.IC (initial condition) commands
■
.INCLUDE (or) .INC (or) .INCL commands
■
.LIB commands
■
.MODEL commands
■
.NODESET commands
■
.OP commands
■
.OPTION (or) .OPTIONS commands
■
.PARAM (or) .PARAMETER (or) .PARAMETERS commands
■
.TEMP (or) .TEMPERATURE commands
■
.TF commands
■
.TRAN commands
■
.VARIATION commands
Caution: When using an .INCLUDE command within an .ALTER
statement, the purpose of this feature is to enable you to slightly
modify the original netlist; perhaps adding some elements/nodes
without changing or deleting any elements/nodes that were
already defined in the original .INC. This feature is not intended
or able to significantly modify elements/nodes to the previously
existing circuit topology. Using .INC statements within an
.ALTER that disregard this limitation will yield simulation results
that are unlikely to reflect the reality of the intended netlist.
Note:
Beginning with the B-2008.09-SP1 release, HSPICE reports the
elapsed time for the top level simulation and each .ALTER block
separately.
Examples
.ALTER simulation_run2
See Also
.OPTION ALTCC
.OPTION MEASFILE
.OPTION OPTCON
Multiprocessing (MP) DC Monte Carlo
34
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.APPENDMODEL
.APPENDMODEL
Appends the .MOSRA (model reliability) parameters to a model card.
Syntax
.APPENDMODEL SrcModel ModelKeyword1 DestModel ModelKeyword2
Argument
Description
SrcModel
Source model name, e.g., the name of the MOSRA model.
ModelKeyword
Model type for SrcModel. For example, the keyword mosra.
DestModel
Destination model name, e.g, the original model in the model library.
ModelKeyword2
Model type for DestModel. For example, 'nmos'.
Description
Appends the parameter values from the source model card (SrcModel) to the
destination model card (DestModel). All arguments are required. Wildcards are
supported for the .APPENDMODEL command. In addition, the .OPTION
APPENDALL enables the top hierarchical level to use the .APPENDMODEL
command even if the MOSFET model is embedded in a subcircuit.
Examples
Example 1
Appending the content of the model card hci_1 to the b3_nch BSIM3
model card.
.appendmodel hci_1 mosra b3_nch nmos
Example 2
Model p1_ra is appended to all of the pmos models. Quotation marks are
required if the model name is defined only by a wildcard.
.appendmodel p1_ra mosra “*” pmos
Example 3
The model p1_ra is appended to all of the pmos models that are named
pch* (pch1, pch2, pch_tt, etc.).
.appendmodel p1_ra mosra pch* pmos
See Also
.MODEL
.MOSRA
.OPTION APPENDALL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
35
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BA_ACHECK
.BA_ACHECK
Specifies the rule for detecting node activity in back-annotation.
Syntax
.BA_ACHECK [include=node_pattern]
+ [exclude=node_pattern]
+ [level=val][level=val2 0|1|n]
+ [dv=val] [start=start_time] [stop=stop_time]
Argument
Description
include=
Defines the signal node name(s) which can be the node name of a single node
node_pattern or a node name containing wildcard character '*' representing a group of node
names. The node name with wildcard character must be quoted by single
quotation marks as 'node_name', because in HSPICE syntax, all characters
after unquoted '*' are treated as comments and are ignored.
exclude=
Defines the signal node name(s) which are excluded from the list of nodes that
node_pattern need to be checked. Wildcard characters can be used and need to be quoted
such as: 'a*'.
level=val
Defines the threshold of voltage variation. A node is considered active when the
voltage change, compared to the initial value of the node, is larger than val.
DEFAULT of val is 0.1 volt.
level=val2
The level value val2 specifies the number of hierarchical depth levels when
checking node activity.
■
■
■
■
dv=val
When val2 is set to 1, only nodes in the root circuit are considered for node
activity.
When val2 is set to n, nodes in the range from the root circuit to nth level
subckt are considered for node activity.
When val2 is set to 0, all subckt levels are considered for node activity.
The default value of val2 is 0.
Defines the threshold of voltage variation. A node is considered active when the
voltage change, compared to the initial value of the node, is larger than val.
DEFAULT of val is 0.1 volt.
start=
Specifies the start_time and stop_time in the time window. The activity is
start_time,
checked at the time within the specified time. If no time window is specified, the
stop= stop_time check is performed from the time 0 ns to the end of simulation.
36
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BA_ACHECK
Description
Use this option to specify the rule for detecting node activity. A node is
considered active if its voltage change exceeds the specified threshold during
the simulation time.
Note:
The .BA_ACHECK command is similar to the HSIM command:
acheck.
See Also
Post-Layout Back-Annotation
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
37
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BIASCHK
.BIASCHK
Monitors the voltage bias, current, device size, expression, and region.
Syntax
As an expression monitor
.BIASCHK 'expression' [limit=lim] [noise=ns]
+ [max=max] [min=min]
+ [simulation=op|dc|tr|all] [monitor=v|i|w|l]
+ [tstart=time1] [tstop=time2] [autostop]
+ [interval=time]
As an element and model monitor
.BIASCHK type terminal1=t1 [terminal2=t2]
+ [limit=lim] [noise=ns] [max=max] [min=min]
+ [simulation=op|dc|tr|all] [monitor=v|i]
+ [name=name1,name2,...]
+ [mname=modname_1,modname_2,...]
+ [tstart=time1] [tstop=time2] [autostop]
+ [except=name_1,name_2,...]
+ [interval=time] [sname=subckt_name1,subckt_name2,...]
As a region monitor
.BIASCHK MOS [region=cutoff|linear|saturation]
+ [simulation=op|dc|tr|all]
+ [name=name1,name2,...]
+ [mname=modname_1,modname_2,...]
+ [tstart=time1] [tstop=time2] [autostop]
+ [except=name1,name2,...]
+ [interval=time] [sname=subckt_name1,subckt_name2,...]
As a length and width monitor
.BIASCHK type monitor=w|l
+ [limit=lim] [noise=ns] [max=max] [min=min]
+ [simulation=op|dc|tr|all]
+ [name=devname_1,devname_2,...]
+ [name=devname_n,devname_n+1,...]
+ [mname=modelname_1,modelname_2,...]
+ [tstart=time1] [tstop=time2] [autostop]
+ [interval=time] [sname=subckt_name1,subckt_name2,...]
38
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BIASCHK
Argument
Description
type
Element type to check. MOS (C, BJT, ...) For a monitor, type can be
DIODE, BIPOLAR, BJT, JFET, MOS, NMOS, PMOS, C, or SUBCKT.
When used with REGION, type can be MOS only.
terminal 1, 2
Terminals between which HSPICE checks (that is, checks between
terminal1 and terminal2):
■
For MOS level 57: nd, ng, ns, ne, np, n6
For MOS level 58: nd, ngf, ns, ngb
■
For MOS level 59: nd, ng, ns, ne, np
■
For other MOS level: nd, ng, ns, nb
■
For capacitor: n1, n2
■
For diode: np, nn
■
For bipolar: nc, nb, ne, ns
■
For JFET: nd, ng, ns, nb
For type=subckt, the terminal names are those pins defined by the
subcircuit definition of mname.
■
limit
Bias check limit that you define. Reports an error if the bias voltage
(between appointed terminals of appointed elements and models) is
larger than the limit.
noise
Bias check noise that you define. The default is 0.1v. Noise-filter some
of the results (the local maximum bias voltage that is larger than the
limit). The next local max replaces the local max if all of the following
conditions are satisfied:local_max-local_min noise. next
local_max-local_min noise. This local max is smaller than the
next local max. For a parasitic diode, HSPICE ignores the smaller local
max biased voltage and does not output this voltage. To disable this
feature, set the noise detection level to 0.
max
Maximum value.
min
Minimum value.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
39
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BIASCHK
Argument
Description
name
Element name to check. If name and mname are not both set for the
element type, the elements of this type are all checked. You can define
more than one element name in keyword name with a comma (,)
delimiter.If doing bias checking for subcircuits:
■
■
■
■
mname
When both mname and name are defined while multiple name
definitions are allowed if a name is also an instance of mname, then
only those names are checked, others will be ignored.
This command is ignored if no name is an instance of mname.
For name definitions which are not of the type defined in mname
will be ignored.
If a mname is not defined, the subcircuit type is determined by the
first name definition.
Model name. If you are doing bias checking for a subcircuit, it is the
subcircuit definition name. HSPICE checks elements of the model for
bias. If you define mname, then HSPICE checks all devices of this
model. You can define more than one model name in the keyword
mname with the comma (,) delimiter. If mname and name are not both
set for the element type, the elements of this type are all checked. If
doing bias checking for subcircuits:
■
Once there is one and only one mname defined, the terminal
names for this command are those pins defined by the subckt
definition of mname.
■
Multiple mname definitions are not allowed.
■
Wildcards are supported for mname.
■
If only mname is specified in a subckt bias check, then all
subcircuits will be checked.
See also sname below.
40
region
Values can be cutoff, linear, or saturation. HSPICE monitors when the
MOS device, defined in the .BIASCHK command, transitions to and
from the specified region (such as cutoff).
simulation
Simulation type you want to monitor. You can specify op, dc, tr
(transient), and all (op, dc, and tr). The tr option is the default
simulation type.
monitor
Type of value you want to monitor. You can specify v (voltage), i
(current), w, and l (device size) for the element type. This parameter is
not used for an expression-type monitor.
tstart
Bias check start time during transient analysis. The default is 0.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BIASCHK
Argument
Description
tstop
Bias check end time during transient analysis. The analysis ends on
its own by default if you do not set this parameter.
autostop
When set, HSPICE supports an autostop for a biaschk card so that it
can report error messages and stop the simulation immediately.
except
Specify the element or instance that you do not want to bias check.
interval
Active when .OPTION BIASINTERVAL is set to a nonzero value. This
argument prevents reporting intervals that are less than or equal to the
time specified.
sname
Name of the subcircuit definition that the type of element of lies in.
HSPICE checks all elements in this subcircuit for bias. You can define
more than one subcircuit name in the keyword sname with a comma
(,) delimiter. If you are doing bias checking for a subcircuit, sname =
the X-element name.
Description
Use this command to monitor the voltage bias, current, device size, expression,
and region during analysis. The output reports:
■
Element (instance) name
■
Time
■
Terminals
■
Bias that exceeds the limit
■
Number of times the bias exceeds the limit for an element
HSPICE saves the information as both a warning and a bias check summary in
the *.lis file or a file you define in the BIASFILE option. You can use this
command only for active elements, capacitors, and subcircuits.
More than one simulation type or all simulation types can be set in a
single .BIASCHK command. Also, more than one region can be set in a
single .BIASCHK command.
After a simulation that uses the .BIASCHK command runs, HSPICE outputs a
results summary including the element name, time, terminals, model name,
and the number of times the bias exceeded the limit for a specified element.
The keywords name, mname, and sname act as OR'd filters for element
selection. Also, if type is subckt in a .BIASCHK command that tries to check
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
41
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BIASCHK
the ports of a subcircuit, the keyword sname then behaves identically to the
name keyword.
Element and model names can contain wildcards, either “?” (stands for one
character) or “*” (stands for 0 or more characters).
If a model name that is referenced in an active element command contains a
period (.), then .BIASCHK reports an error. This occurs because it is unclear
whether a reference such as x.123 is a model name or a subcircuit name (123
model in “x” subcircuit).
If you do not specify an element and model name, HSPICE checks all elements
of this type for bias voltage (you must include type in the BIASCHK card).
However, if type is subckt at least one element or model name must be
specified in the .BIASCHK command; otherwise, a warning message is issued
and this command is ignored.
Note:
To perform a complete bias check and print all results in the
Outputs Biaschk Report, do not use .protect/.unprotect in
the netlist for the part that is used in .biaschk. For example: If
a model definition such as model nch is contained within
.prot/.unprot commands, in the *.lis you'll see a warning
message as follows: **warning** : model nch defined
in .biaschk cannot be found in netlist--ignored
Examples
Example 1
Monitoring an expression:
.biaschk 'v(1)' min='v(2)*2' simulation= op
Example 2
Monitoring element m1 and model types between two specified
terminals.
.biaschk nmos terminal1=ng terminal2=ns simulation=tr name=m1
Example 3
Monitoring MOSFET model m1 whose bias voltage exceeds 2.5 V and
interval exceeds 5 ns.
.biaschk nmos terminal1=nb terminal2=ng limit=2.5
+ mname=m1 interval=5n
Example 4
The following two examples use .BIASCHK commands that do not
require terminal specifications. Example 4 monitors the MOS transistor
region of operation
.biaschk mos region=saturation name=x1.m1 mname=nch name=m2
42
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.BIASCHK
Example 5
Monitors MOS transistor length and width.
.biaschk mos monitor=l mname=m* p* min=1u minu=op
Example 6
Defines the differences between using .BIASCHK with a MOSFET
instance and macro models. If the MOSFET in your netlist is written as
follows:
mp0 gd s sub dgxnfet w=1.0u l=0.18u
...then the .BIASCHK statement can be written as:
.biaschk pmos terminal1=ns terminal2=nd mname=m*.dgnfet*
+ limit=0.9v
Example 7
If a macro model is used, then the MOSFET is defined inside a subcircui:
.subckt test g d
mp0 g d s sub dgxnfet w=1.0u l=0.18u
.model dgxnfet nmos level=54
.ends
X1 g d test
For this case
.biaschk pmos terminal1=ns terminal2=nd mname=x*.dgnfet*
+ limit=0.9v
For a full example netlist go to:$installdir/demo/hspice/apps/biaschk.sp
See Also
.OPTION BIASFILE
.OPTION BIASINTERVAL
.OPTION BIASNODE
.OPTION BIASPARALLEL
.OPTION BIAWARN
.PROTECT or .PROT
.UNPROTECT or .UNPROT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
43
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CFL_PROTOTYPE
.CFL_PROTOTYPE
Specifies function protocol type for the Compiled Function Library capability.
Syntax
.CFL_PROTOTYPE function_name(arg1_type, arg2 type,...,argn
type)
Argument
Description
function_name
CFL function name
arg_type
input argument type; it can be
■
■
double: (default) keyword argument passed to C library as C
language's “double” type for C code used in C-based file (not
HSPICE netlist); used to generate the *.so file (CFL library file)
param: parameter storage reference as output only
Description
This command specifies a function type.
Function types include:
■
a predefined parameter value
■
a mathematical expression of multiple predefined parameter values
■
a built-in mathematical function in the standard library
■
an output of another evaluated CFL function
The CFL function can re-assign local and global parameter values. Only local
functions with the parameters in the argument list are updated with the new
local values. The global functions are updated with the new global values.
The following rules apply:
44
■
CFL functions cannot be used in .PRINT, .PROBE and .MEASURE
statements.
■
Only a single compiled CFL *.so file is allowed in the simulation input netlist.
■
Parameter definition must be order-dependent when using multiple return
values for the CFL functions (unlike the current HSPICE order-independent
parameter definition requirement).
■
If the CFL function name is same as the user-defined function (UDF), the
UDF is used and CFL is not called.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CFL_PROTOTYPE
Note:
In the C code, the protocol type of C library must be
func(argc,argv), where argc is argument number, and
argv is the argument array. See Examples 2 and 3 for sample
CFL function syntax.
The CFL feature requires setting an environment variable,
CFL_COMPILED_LIB CFL_library_file_name, (*.so file) and use of the
.OPTION CFLFLAG to enable it in a netlist. For other descriptive information on
the Compiled Library Function see Features in the HSPICE User Guide:
Simulation and Analysis.
Examples
Example 1
Note the use of the “&” notation that signifies the bidirectional nature of
an argument which means the value of the argument is updated upon
returning from the function. The example presents multiple return values
for the CFL functions:
.CFL_PROTOTYPE xyz_eval (double, param)
.param p1=5
.param p2=9
.param p3= xyz_eval(p1, &p2)
Example 2
In this Sample CFL function, the content of the “return” parameters
does not affect the calculated return values from the function with
the same arguments. Parameters passed into the functions as
references are used only as return values and do not contribute to
the calculation inside the CFL function in any form.
double func1 (int argc, long **argv)
{
double a1 = *(double*)argv[0];
double *a2 = (double*)argv[1];
return eval1_func(a1, a2);
}
double eval1_func (double arg1, double *arg2)
{
double val = 0;
*arg2 = arg1 + 2;
val = (*arg2) * (arg1 + 4)
return val
}
In Example 2, CFL C-code Function Implementation, CFL functions are an
arbitrary number of function arguments with any combination of the argument
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
45
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CFL_PROTOTYPE
base type as either “double” or parameter address. Example 3 is the function
prototype:
Example 3
Netlist Showing Redefinition of User Functions
static double
eval1_func(double a1, double *a2)
{
*a2 = a1 + 10;
return a1 - 4;}
double xyz_eval 1(int argc, long **argv)
{
double a1 = *(double *)(argv[0]);
double *a2 = (double*)argv[1];
return eval1_func(a1, a2);
}
static double
eval2_func(double *a1, double a2, double *a3)
{
*a1 = a2 + 2;
*a3 = a2 - 3;
return a2 - 1;
}
double xyz_eval_2(int argc, long **argv)
{
double *a1 = (double*)(argv[0]);
double a2 = *(double *)argv[1];
double *a3 = (double *)argv[2];
return eval2_func(a1, a2, a3);
}
Example 4
.param p2
.param p1
.param p3
Redefinition following evaluations
= 10
= 2
= func1 (p1, &p2)
After returning from evaluating func1(), p3=24, and user function are
redefined to p2=4.
.subckt INV
.param p1 = 3
.param p2 = 3
.param p3 = func1(p1, &p2)
46
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CFL_PROTOTYPE
After returning from evaluating func1(), the user function p1=3 is redefined
to p2=5 while p3=35.
.param p3 = 0
.param p4 = func1(p2, &p3)
After the evaluation of func1(), p2=5 and p3=7 & p4=63.
.ends INV
Example 5
Sample Netlist
*
.cfl_prototype zyz_eval_1(double, param)
.cfl_prototpye xyz_eval_2(param, double, param)
*
.param p1 = 5
.param p2 = 8
.param p3 = 9
.param p4 = 7
.param p5 = 10
*
.param p7 = xyz_eval_1(p1, &p2)
* p2 = 15 ; p7 = 1
.param p8 = xyz_eval_2(&p3, p4, &p5) * p3 = 9; p5 = 4; p8 = 6
.param p9 = p8 + p5 - p3 + p2
*
R1 n1 A r="p2"
* R = 15
R2 n3 B r="p7"
* R = 1
M1 n1 n2 n3 NMOS w=5u l=6u bqi="p9"
* bqi = 16
See Also
.OPTION CFLFLAG
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
47
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK EDGE
.CHECK EDGE
Verifies that a triggering event provokes an appropriate RISE or FALL action in
HSPICE RF.
Syntax
.CHECK EDGE (ref RISE | FALL minmax RISE | FALL)
+ node1 [node2 ...] (hi lo hi_th low_th)
Argument
Description
ref
Name of the reference signal.
min
Minimum time.
max
Maximum time.
node1 node2 ...
List of nodes to which you apply the edge condition.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use a .CHECK EDGE command to verify that a triggering event provokes an
appropriate RISE or FALL action within the specified time window.
Examples
This example sets the condition that the rising action of the clock (clk) triggers
the falling edge of VOUTA within 1 to 3 ns, as shown in Figure 1:
.CHECK EDGE (clk RISE 1ns 3ns FALL) VOUTA
Values for hi, lo, and the thresholds were defined in a .CHECK GLOBAL_LEVEL
command placed earlier in the netlist.
voutA
CLK
HI
HI_thresh
LO_thresh
LO
1ns < t < 3 ns
Figure 1
48
EDGE Example
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK EDGE
See Also
.CHECK HOLD
.CHECK GLOBAL_LEVEL
.CHECK SETUP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
49
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK FALL
.CHECK FALL
Verifies that a fall time occurs within a specified time window in HSPICE RF.
Syntax
.CHECK FALL (minmax) node1 [node2 ...]
(hi lo hi_th lo_th)
Argument
Description
min
Lower boundary for the time window.
max
Upper limit for the time window.
node1 node2 ...
List of all nodes to check.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use a .CHECK FALL command verifies that a fall time occurs within the
specified window of time.
See Also
.CHECK GLOBAL_LEVEL
.CHECK RISE
.CHECK SLEW
50
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK GLOBAL_LEVEL
.CHECK GLOBAL_LEVEL
Globally sets specified high and low definitions for all CHECK commands in
HSPICE RF.
Syntax
.CHECK GLOBAL_LEVEL (hi lo hi_th lo_th)
Argument
Description
hi
Value for logic high.
lo
Value for logic low.
hi_th
Is the minimum value considered high.
lo_th
Is the maximum value considered low.
Description
Use this command to globally set the desired high and low definitions for all
CHECK commands. The high and low definitions can be either numbers or
expressions, and hi_th and lo_th can be either absolute values or percentages
if punctuated with the % symbol. You can also locally set different logic levels
for individual timing checks.
Examples
Example 1
Defines a logic high as 5 volts and a logic low as 0 volts. A voltage value
as small as 4 V is considered high, while a value up to 1 V is low.
.CHECK GLOBAL_LEVEL (5 0 4 1)
Example 2
Illustrates an alternative definition for the first example.
.CHECK GLOBAL_LEVEL (5 0 80% 20%)
See Also
.CHECK EDGE
.CHECK FALL
.CHECK HOLD
.CHECK IRDROP
.CHECK RISE
.CHECK SLEW
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
51
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK HOLD
.CHECK HOLD
Ensures that specified signals do not switch for a specified period of time in
HSPICE RF.
Syntax
.CHECK HOLD (ref RISE | FALL duration RISE | FALL)
+ node1 [node2 ...] (hi lo hi_th low_th)
Argument
Description
ref
Reference or trigger signal.
duration
Minimum time required after the triggering event before the
specified nodes can rise or fall.
node1 node2 ...
List of nodes for which the HOLD condition applies.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use this command to ensure that the specified signals do not switch for a
specific period of time.
Examples
This example specifies that vin* (such as vin1, vin2, and so on), must not
switch for 2ns after every falling edge of nodeA (see Figure 2).
.CHECK HOLD (nodeA FALL 2ns RISE) vin*
vin*
nodeA
HI
HI_thresh
LO_thresh
LO
t >=2ns
Figure 2
52
HOLD Example
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK HOLD
See Also
.CHECK EDGE
.CHECK GLOBAL_LEVEL
.CHECK SETUP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
53
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK IRDROP
.CHECK IRDROP
Verifies that IR drop does not fall below or exceed a specified value in HSPICE
RF.
Syntax
.CHECK IRDROP (volt_valtimeduration) node1 [node2 ...]
+ (hi lo hi_th low_th)
Argument
Description
volt_val
Limiting voltage value.
■
■
A positive volt_val (voltage value) indicates ground bounce
checking.
A negative volt_val denotes VDD drop.
duration
Maximum allowable time. If you set duration to 0, then HSPICE
RF reports every glitch that strays beyond the specified volt_val.
node1 [node2 ...]
List of nodes for which the IR drop checking applies.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use this command to verify that the IR drop does not fall below or exceed a
specified value for a specified duration.
Examples
This example specifies that v1 must not fall below -2 volts for any duration
exceeding 1ns (see Figure 3).
.CHECK IRDROP (-2 1ns) v1
v1
-2 volts
t <=1ns
Figure 3
54
IR Drop Example
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK IRDROP
See Also
.CHECK EDGE
.CHECK GLOBAL_LEVEL
.CHECK SETUP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
55
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK RISE
.CHECK RISE
Verifies that a rise time occurs within a specified time window in HSPICE RF.
Syntax
.CHECK RISE (minmax) node1 [node2 ...] (hi lo hi_th lo_th)
Argument
Description
min
Lower boundary for the time window.
max
Upper limit for the time window.
node1 node2 ...
List of all nodes to check.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use this command to verify that a rise time occurs within the specified window
of time.
Examples
This example defines a window between 1.5ns and 2.2ns wide, in which the va
and vb signals must complete their rise transition (see Figure 4). Values for the
HI, LO, and the thresholds were defined in a .CHECK GLOBAL_LEVEL
command placed earlier in the netlist.
.CHECK RISE (1.5ns 2.2ns) va vb
HI
HI_thresh
LO_thresh
LO
1.5 ns < t < 2.2 ns
Figure 4
56
RISE Time Example
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK RISE
See Also
.CHECK GLOBAL_LEVEL
.CHECK FALL
.CHECK SLEW
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
57
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK SETUP
.CHECK SETUP
(RF) Verifies that specified signals do not switch for a specified time-period.
Syntax
.CHECK SETUP (ref RISE | FALL duration RISE | FALL)
+ node1 [node2 ...] (hi lo hi_th low_th)
Argument
Description
ref
Reference or trigger signal.
duration
Minimum time before the triggering event during which the
specified nodes cannot rise or fall
node1 [node2 ...]
List of nodes for which the HOLD condition applies.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use to verify that specified signals do not switch for a specified period of time.
Examples
This example specifies that v1 and v2 must not switch for 2 ns before every
rising edge of nodeA (see Figure 5).
.CHECK SETUP (nodeA RISE 2ns FALL) v1 v2
nodeA
v1
HI
HI_thresh
LO_thresh
LO
t >=2ns
Figure 5
SETUP Example
See Also
.CHECK EDGE
.CHECK GLOBAL_LEVEL
.CHECK HOLD
58
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK SLEW
.CHECK SLEW
Verifies that a slew rate occurs within a specified time window in HSPICE RF.
Syntax
.CHECK SLEW (minmax) node1 [node2 ...](hi lo hi_th lo_th)
Argument
Description
min
Lower boundary for the time window.
max
Upper limit for the time window.
node1 node2 ...
List of all nodes to check.
hi lo hi_th lo_th
Logic levels for the timing check.
Description
Use this command to verify that a slew rate occurs within specified time range.
Examples
This example sets the condition that nodes starting with a* nodes must have a
slew rate between (HI_thresh - LO_thresh)/3ns and (HI_thresh - LO_thresh)/
1ns. If either node has a slew rate greater than that defined in the .CHECK
SLEW command, HSPICE RF reports the violation in the .err file.
.CHECK SLEW (1ns 3ns) a* (3.3 0 2.6 0.7)
The slew rate check in Figure 6 defines its own hi, lo, and corresponding
threshold values, as indicated by the four values after the node names.
3.3
2.6
0.7
0.0
1ns < t < 3ns
Figure 6
SLEW Example
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
59
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CHECK SLEW
See Also
.CHECK FALL
.CHECK GLOBAL_LEVEL
.CHECK RISE
60
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CONNECT
.CONNECT
Connects two nodes together; the first node replaces the second node in the
simulation.
Syntax
.CONNECT node1node2
Argument
Description
node1
Name of the first of two nodes to connect together
node2
Name of the second of two nodes to connect together. This node is
replaced by Node1, which is the first node, in the simulation.
Description
Use this command to connect two nodes together in your netlist. This causes
the simulation to evaluate the two nodes as if they were only one node that
uses the name of the first node. The name of the second node is not
recognized in the simulation. Both nodes must be at the same level in the circuit
design that you are simulating: you cannot connect nodes that belong to
different subcircuits.
A .CONNECT statement in the higher level does not work on the .SUBCKT
node.
Examples
Example 1
A is the name of the first of two nodes to connect together and VSS
is the name of the second of two nodes to connect together. A, the
first node, replaces the second node, VSS, in the simulation.
.CONNECT A VSS
...
.subckt eye_diagram node1 node2 ...
.connect node1 node2
...
.ends
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
61
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CONNECT
Example 2
Example 1 now is the same as the following:
...
.subckt eye_diagram node1 node1 ...
...
.ends
...
HSPICE reports the following error message:
**error**: subcircuit definition duplicates node node1
To apply any HSPICE command to node2, apply it to node1, instead. Then, to
change the netlist construction to recognize node2, use an .ALTER command.
HSPICE reports the following error message:
**error**: subcircuit definition duplicates node node1
To apply any HSPICE command to node2, apply it to node1, instead. Then, to
change the netlist construction to recognize node2, use an .ALTER command.
In the following variation of the example, node1 node2 are not be the same in
this situation and the duplicated node error message will not be issued.
.connect node1 node2
.subckt eye_diagram node1 node2 ...
...
.ends
Example 3
The first .TRAN simulation includes two resistors. Later simulations have
only one resistor because r2 is short-circuited by connecting cc with 1.
v(1) does not print out, but v(cc) prints out instead.
*example for .connect
vcc 0 cc 5v
r1 0 1 5k
r2 1 cc 5k
.tran 1n 10n
.print i(vcc) v(1)
.alter
.connect cc 1
.end
Example 4
62
Shows how to use multiple .CONNECT commands to connect several
nodes together. This example connects both node2 and node3 to node1.
All connected nodes must be in the same subcircuit or all in the main
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.CONNECT
circuit. The first HSPICE simulation evaluates only node1; node2 and
node3 are the same node as node1. Use .ALTER commands to simulate
node2 and node3.
.CONNECT node1 node2
.CONNECT node2 node3
If you set .OPTION NODE, then HSPICE prints out a node connection table.
vcc cc 0 5v
r1 cc net1 5k
r2 net1 net2 5k
c1 net2 0 1n
.tran 1n 10n
.connect net2 0
.print i(vcc) v(net2)
.end
This causes the circuit elements to be connected as shown in Example 5:
Example 5
vcc cc net2 5v
r1 cc net1 5k
r2 net1 net2 5k
c1 net2 net2 1n
.tran 1n 10n
.connect net2 0
.print i(vcc) v(net2)
.end
For Example 5, HSPICE reports the following error message for the elements
vcc r1 and r2, since there is now no ground node in the netlist.
**error** no dc path to ground from node
Example 6
The correct way to connect net2 to ground is to specify the .CONNECT
command as follows:
.connect 0 net2
See Also
.ALTER
.OPTION NODE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
63
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
.DATA
Concatenates or column-laminates data sets to optimize measured I-V, C-V,
transient, or S-parameter data.
Syntax
Inline command
.DATA datanm pnam1 [pnam2 pnam3 ... pnamxxx]
+
pval1 [pval2 pval3 ... pvalxxx]
+
pval1’ [pval2’ pval3’ ... pvalxxx’]
.ENDDATA
External File command for concatenated data files
.DATA datanm MER
+ FILE=’filename1’ pname1=col_num [pname2=col_num ...]
+ [FILE=’filename2’ pname1=col_num
+ [pname2=col_num ...] ... [OUT=’fileout’]
.ENDDATA
Column Laminated command (not available for HSPICE RF)
.DATA datanm LAM
+ FILE=’filename1’ pname1=col_num
+ [pname2=col_num ...]
+ [FILE=’filename2’ pname1=col_num
+ pname2=col_num ...] ... [OUT=’fileout’]
.ENDDATA
64
Argument
Description
col_num
Column number in the data file for the parameter value. The column
does not need to be the same between files.
datanm
Data name—referenced in the .TRAN, .DC, or .AC command.
filenamei
Data file to read. HSPICE concatenates files in the order they appear
in the .DATA command. You can specify up to 10 files.
fileouti
Data file name, where simulation writes concatenated data. This file
contains the full syntax for an inline .DATA command and can replace
the .DATA command that created it in the netlist. You can output the
file and use it to generate one data file from many.
LAM
Column-laminated (parallel merging) data files to use.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
Argument
Description
MER
Concatenated (series merging) data files to use.
pnami
Parameter names—used for source value, element value, device size,
model parameter value, and so on. You must declare these names in
a .PARAM command.
pvali
Parameter value.
Description
Use the .DATA command to concatenate or column-laminate data sets to
optimize measured I-V, C-V, transient, or S-parameter data.
You can also use the .DATA command for a first or second sweep variable
when you characterize cells and test worst-case corners. Simulation reads data
measured in a lab, such as transistor I-V data, one transistor at a time in an
outer analysis loop. Within the outer loop, the analysis reads data for each
transistor (IDS curve, GDS curve, and so on), one curve at a time in an inner
analysis loop.
Data-driven analysis syntax requires a .DATA command and an analysis
command that contains a DATA=dataname keyword.
The .DATA command specifies parameters that change values, and the sets of
values to assign during each simulation. The required simulations run as an
internal loop. This bypasses reading-in the netlist and setting-up the simulation,
which saves computing time. In internal loop simulation you can also plot
simulation results against each other and print them in a single output.
You can enter any number of parameters in a .DATA block. The .AC, .DC,
and .TRAN commands can use external and inline data provided in .DATA
commands. For example, to specify the circuit temperature for an HSPICE
simulation you can use the .TEMP command, the TEMP parameter in the .DC,
.AC, and .TRAN commands, or the TEMP/TEMPER parameter in the first
column of the .DATA command.The number of data values per line does not
need to correspond to the number of parameters. For example, you do not
need to enter 20 values on each line in the .DATA block if each simulation pass
requires 20 parameters: the program reads 20 values on each pass, however
the values are formatted.
Each .DATA command can contain up to 50 parameters. If you need more than
50 parameters in a single .DATA command, place 50 or less parameters in
the .DATA command, and use .ALTER commands for the other parameters.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
65
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
HSPICE refers to .DATA commands by their data names so each data name
must be unique. HSPICE supports three .DATA command formats:
■
Inline data, which is parameter data, listed in a .DATA command block. The
datanm parameter in a .DC, .AC, or .TRAN analysis command, calls this
command. The number of parameters that HSPICE reads determines the
number of columns of data. The physical number of data numbers per line
does not need to correspond to the number of parameters. For example, if
the simulation needs 20 parameters you do not need 20 numbers per line.
■
Data that is concatenated from external files. Concatenated data files are
files with the same number of columns, placed one after another.
■
Data that is column-laminated from external files. Column laminated data
are columns of files with the same number of rows, arranged side-by-side.
To use external files with the .DATA format:
■
Use the MER and LAM keywords to prepare HSPICE for external file data,
rather than inline data.
■
Use the FILE keyword to specify the external filename.
■
Use simple file names, such as out.dat without single or double quotation
marks ( ‘ ’ or “ ”), but use quotation marks when file names start with
numbers, such as “1234.dat”.
■
Use the proper case, since file names are case sensitive on UNIX systems.
For data-driven analysis, specify the start time (time 0) in the analysis
command so that the analysis correctly calculates the stop time.
The following shows how different types of analyses use .DATA
commands: .DC DATA=dataname
Operating point: .DC vin 1 5 .25 SWEEP DATA=dataname
DC sweep:
.DC vin 1 5 .25 SWEEP DATA=dataname
AC sweep:
AC dec 10 100 10meg SWEEP DATA=dataname
TRAN sweep:
.TRAN 1n 10n SWEEP DATA=dataname
Examples
Example 1
66
HSPICE performs these analyses for each set of parameter values
defined in the .DATA command. For example, the program first uses the
width=50u, length=30u, thresh=1.2v, and cap=1.2pf parameters to
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
perform .TRAN, .AC, and .DC analyses. HSPICE then repeats the
analyses for width=25u, length=15u, thresh=1.0v, and cap=0.8pf, and
again for the values on each subsequent line in the .DATA block.
* Inline .DATA statement
.TRAN
1n
100n
SWEEP DATA=devinf
.AC DEC
10
1hz
10khz
SWEEP DATA=devinf
.DC TEMP
-55
125
10
SWEEP DATA=devinf
.DATA
devinf
width
length
thresh
cap
+
50u
30u
1.2v
1.2pf
+
25u
15u
1.0v
0.8pf
+
5u
2u
0.7v
0.6pf
.ENDDATA
Example 2
HSPICE performs a DC sweep analysis for each set of VBS, VDS,
and L parameters in the .DATAvdot block. That is, HSPICE runs
eight DC analyses one for each line of parameter values in
the .DATA block.
* .DATA as the inner sweep
M1 1 2 3 0 N
W=50u
L=LN
VGS 2 0 0.0v
VBS 3 0 VBS
VDS 1 0 VDS
.PARAM VDS=0 VBS=0 L=1.0u
.DC DATA=vdot
.DATA vdot
VBS
VDS
L
0
0.1
1.5u
0
0.1
1.0u
0
0.1
0.8u
-1
0.1
1.0u
-2
0.1
1.0u
-3
0.1
1.0u
0
1.0
1.0u
0
5.0
1.0u
.ENDDATA
Example 3
These values result in transient analyses at every time value from 0 to
100 ns in steps of 1 ns by using the first set of parameter values in
the .DATA d1 block. Then HSPICE reads the next set of parameter values
and does another 100 transient analyses. It sweeps time from 0 to 100
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
67
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
ns in 1 ns steps. The outer sweep is time and the inner sweep varies the
parameter values. HSPICE performs 200 analyses: 100 time increments,
times 2 sets of parameter values.
* .DATA as the outer sweep
.PARAM W1=50u W2=50u L=1u CAP=0
.TRAN 1n 100n SWEEP DATA=d1
.DATA d1
W1
W2
L
CAP
50u
40u
1.0u
1.2pf
25u
20u
0.8u
0.9pf
.ENDDATA
Example 4
This example shows the external file .DATA for concatenated data files.
* External File .DATA for concatenated data files
.DATA datanm MER
+ FILE=filename1 pname1 = colnum
+ pname2=colnum ...
+ FILE=filename2 pname1=colnum
+ pname2=colnum ...
+ ...
+ OUT=fileout
.ENDDATA
If you concatenate the three files (file1, file2, and file3).
file1
a a a
a a a
a a a
file2
b b b
b b b
file3
c c c
c c c
The data appears as follows:
Example 5
a a a
a a a
a a a
b b b
b b b
c c c
c c c
The number of lines (rows) of data in each file does not need to be the same.
The simulator assumes that the associated parameter of each column of the A
68
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
file is the same as each column of the other files. The .DATA command for this
example is:
* External File
.DATA inputdata
FILE=‘file1’
FILE=‘file2’
FILE=‘file3’
.ENDDATA
.DATA statement
MER
p1=1 p2=3 p3=4
p1=1
This example listing concatenates file1, file2, and file3 to form the inputdata
data set. The data in file1 is at the top of the file, followed by the data in file2,
and file3. The inputdata in the .DATA command references the data name
specified in either the .DC, .AC, or .TRAN analysis commands. The parameter
fields specify the column that contains the parameters (you must already have
defined the parameter names in .PARAM commands). For example, the values
for the p1 parameter are in column 1 of file1 and file2. The values for the p2
parameter are in column 3 of file1. For data files with fewer columns than
others, HSPICE assigns values of zero to the missing parameters.
(HSPICE only) In Example 5 three files (D, E, and F) contain the following
columns of data:
Example 6
File D
File E
d1 d2 d3
e4 e5
d1 d2 d3
e4 e5
d1 d2 d3
e4 e5
File F
f6
f6
f6
The laminated data appears as follows:
d1 d2 d3
d1 d2 d3
d1 d2 d3
e4 e5
e4 e5
e4 e5
f6
f6
f6
The number of columns of data does not need to be the same in the three files.
The number of lines (rows) of data in each file does not need to be the same.
HSPICE interprets missing data points as zero.
The .DATA command for this example is:
* Column-Laminated .DATA statement
.DATA dataname LAM
FILE=‘file1’ p1=1 p2=2 p3=3
FILE=‘file2’ p4=1 p5=2
OUT=‘fileout’
.ENDDATA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
69
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DATA
This listing laminates columns from file1 and file2 into the fileout output file.
Columns one, two, and three of file1 and columns one and two of file2 are
designated as the columns to place in the output file. You can specify up to 10
files per .DATA command.
If you run HSPICE on a different machine than the one on which the input data
files reside (such as when you work over a network), use full path names
instead of aliases. Aliases might have different definitions on different
machines.
See Also
.AC
.DC
.ENDDATA
.PARAM (or) .PARAMETER (or) .PARAMETERS
.TRAN
70
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DC
.DC
Performs several types of sweeps during DC analysis.
Syntax
Sweep or Parameterized Sweep:
.DC var1 START=start1 STOP=stop1 STEP=incr1
.DC var1 START=[param_expr1]
+ STOP=[param_expr2] STEP=[param_expr3]
.DC var1 start1 stop1 incr1
+ [SWEEP var2 type np start2 stop2]
.DC var1 start1 stop1 incr1 [var2 start2 stop2 incr2]
Data-Driven Sweep:
.DC var1 type np start1 stop1 [SWEEP DATA=datanm]
.DC DATA=datanm [SWEEP var2 start2 stop2 incr2]
.DC DATA=datanm
Monte Carlo:
.DC var1 type np start1 stop1 [SWEEP MONTE=MCcommand]
.DC MONTE=MCcommand
Optimization:
.DC DATA=datanm OPTIMIZE=opt_par_fun
+ RESULTS=measnames MODEL=optmod
.DC var1 start1 stop1 SWEEP OPTIMIZE=OPTxxx
+ RESULTS=measname MODEL=optmod
Argument
Description
DATA=datanm Datanm is the reference name of a .DATA command.
incr1...
Voltage, current, element, or model parameters; or temperature
increments.
MODEL
Optimization reference name. The .MODEL OPT command uses this
name in an optimization analysis
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
71
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DC
Argument
Description
MONTE=
MCcommand
Where MCcommand can be any of the following:
■
■
■
■
np
Number of points per decade or per octave or just number of points,
based on which keyword precedes it.
OPTIMIZE
Specifies the parameter reference name, used for optimization in
the .PARAM command
RESULTS
Measure name used for optimization in the .MEASURE command
start1 ...
Starting voltage, current, element, or model parameters; or
temperature values. If you use the POI (list of points) variation type,
specify a list of parameter values, instead of start stop.HSPICE
supports the start and stop syntax; HSPICE RF does not.
stop1 ...
Final voltage, current, any element, model parameter, or temperature
values.
SWEEP
Second sweep has a different type of variation (DEC, OCT, LIN, POI,
or DATA command; or MONTE=val).
TEMP
Temperature sweep.
type
Can be any of the following keywords:
■
■
■
■
72
val Specifies the number of random samples to produce.
val firstrun=num Specifies the sample number on which the
simulation starts.
list num Specifies the sample number to execute.
list(num1:num2 num3 num4:num5) Samples from num1 to num2,
sample num3, and samples from num4 to num5 are executed
(parentheses are optional).
DEC — decade variation
OCT — octave variation
LIN — linear variation
POI — list of points
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DC
Argument
Description
var1 ...
■
Name of an independent voltage or current source, or
Name of any element or model parameter, or
■
TEMP keyword (indicating a temperature sweep).
HSPICE supports a source value sweep, which refers to the source
name (SPICE style). However, if you select a parameter sweep,
a .DATA command, and a temperature sweep, then you must select
a parameter name for the source value. A later .DC command must
refer to this name. The parameter must not start with the TEMP
keyword. The var1 parameter should be defined in advance using
the.PARAM command.
■
firstrun
The val value specifies the number of Monte Carlo iterations to
perform. The firstrun value specifies the desired number of iterations.
HSPICE runs from num1 to num1+val-1.
list
The iterations at which HSPICE performs a Monte Carlo analysis. You
can write more than one number after list. The colon represents
“from ... to ...". Specifying only one number makes HSPICE run at
only the specified point.
Description
You can use the .DC command in DC analysis to:
■
Sweep any parameter value.
■
Sweep any source value.
■
Sweep temperature range.
■
Perform a DC Monte Carlo (random sweep) analysis.
■
Perform a data-driven sweep.
■
Perform a DC circuit optimization for a data-driven sweep.
■
Perform a DC circuit optimization by using start and stop.
■
Perform a DC model characterization.
The format for the .DC command depends on the application that uses it. The
DC sweep functionality is enhanced by use of the GSHUNT algorithm.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
73
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DC
Examples
Example 1
Sweeps the value of the VIN voltage source from 0.25 volts to 5.0 volts in
increments of 0.25 volts.
.DC VIN 0.25 5.0 0.25
Example 2
Sweeps the drain-to-source voltage from 0 to 10 v in 0.5 v increments at
VGS values of 0, 1, 2, 3, 4, and 5 v.
.DC VDS 0 10 0.5 VGS 0 5 1
Starts a DC analysis of the circuit from -55° C to 125° C in 10° C
increments.
.DC TEMP -55 125 10
Example 3
Example 4
Script runs a DC analysis at five temperatures: 0, 30, 50, 100, and 125
° C.
.DC XVAL 1K 10K .5K SWEEP TEMP LIN 5 25 125
Example 5
Runs a DC analysis on the circuit at each temperature value. The
temperatures result from a linear temperature sweep from 25° C to
125° C (five points), which sweeps a resistor value named xval from 1 k
to 10 k in 0.5 k increments.
.DC XVAL 1K 10K .5K SWEEP TEMP LIN 5 25 125
Example 6
Specifies a sweep of the par1 value from 1 k to 100 k in increments of 10
points per decade.
.DC DATA=DATANM SWEEP PAR1 DEC 10 1K 100K
Example 7
Requests a DC analysis at specified parameters in the .DATA DATANM
command. It also sweeps the par1 parameter from 1k to 100k in
increments of 10 points per decade.
.DC PAR1 DEC 10 1K 100K SWEEP DATA=DATANM
Example 8
Invokes a DC sweep of the par1 parameter from 1k to 100k by 10 points
per decade by using 30 randomly generated (Monte Carlo) values.
.DC PAR1 DEC 10 1K 100K SWEEP MONTE=30
74
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DC
Example 9
Schmitt Trigger script.
*file: bjtschmt.sp
bipolar schmitt trigger
.OPTION post=2
vcc 6 0 dc 12
vin 1 0 dc 0 pwl(0,0 2.5u,12 5u,0)
cb1 2 4 .1pf
rc1 6 2 1k
rc2 6 5 1k
rb1 2 4 5.6k
rb2 4 0 4.7k
re 3 0 .47k
diode 0 1 dmod
q1 2 1 3 bmod 1 ic=0,8
q2 5 4 3 bmod 1 ic=.5,0.2
.dc vin 0,12,.1
.model dmod d is=1e-15 rs=10
.model bmod npn is=1e-15 bf=80 tf=1n
+ cjc=2pf cje=1pf rc=50 rb=100 vaf=200
.probe v(1) v(5)
.print
.end
Example 10 Invokes a DC sweep of the par1 parameter from 1k to 100k by 10 points
per decade and uses 10 Monte Carlo) values from 11th to 20th trials.
.DC par1 DEC 10 1k 100k SWEEP MONTE=list(10 20:30 35:40 50)
Example 11 Invokes a DC sweep of the par1 parameter from 1k to 100k by 10 points
per decade and a Monte Carlo analysis at the 10th trial, then from the
20th to the 30th trials, followed by the 35th to 40th trials and finally at the
50th trial.
.DC par1 DEC 10 1k 100k SWEEP MONTE=list(10 20:30 35:40 50)
See Also
.MODEL
.OPTION DCIC
.PARAM (or) .PARAMETER (or) .PARAMETERS
Behavioral Application Examples for the path to the demo file
inv_vin_vout.sp
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
75
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DCMATCH
.DCMATCH
Calculates the effects of variations on a circuit's DC characteristics.
Syntax
.DCMATCH OUTVAR [THRESHOLD=T] [FILE=string] [INTERVAL=Int]
Argument
Description
OUTVAR
One or more node voltages, voltage differences for a node pair, or
currents through an independent voltage source or currents through
a resistor, a capacitor, or an inductor.
THRESHOLD
Report devices with a relative contribution above Threshold in the
summary table.
■
T=0: reports results for all devices
T<0: suppresses table output; however, individual results are still
available through .PROBE or .MEASURE commands.
The upper limit for T is 1, but at least 10 devices are reported or all if
there are less than 10. Default value is 0.01.
■
FILE
Valid file name for the output tables. Default is basename.dm# where
“#” is the usual sequence number for HSPICE output files.
INTERVAL
Applies only if a DC sweep is specified. Int is a positive integer. A
summary is printed at the first sweep point, then for each subsequent
increment of Int and then if not already printed at the final sweep point.
Only single sweeps are supported.
Description
Use this command to calculate the effects of variations in device characteristics
on the DC solution of a circuit.
You can perform only one DCMATCH analysis per simulation. Only the last
.DCMATCH command is used in case more than one in present. The others are
discarded with warnings.
Examples
Example 1
HSPICE reports DCmatch variations on the voltage of node 9, the
voltage difference between nodes 4 and 2, and on the current through the
source VCC and on the current through resister x1.r1.
.DCMatch V(9) V(4,2) I(VCC) I(x1.r1)
76
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DCMATCH
Example 2
The variable XVal is being swept in the .DC command. It takes nine
values in sequence from 1k to 9k in increments of 1k. Tabular output for
the.DCMATCH command is only generated for the set XVal={1k, 4k, 7k,
9k}.
.DC XVal Start=1K Stop=9K Step=1K
.DCMATCH V(vcc) interval=3
See Also
.DC
.MEASURE (DCMATCH)
.PROBE
DCMatch Analysis
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
77
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DCSENS
.DCSENS
Invokes DC sensitivity analysis using variation definitions as specified in the
Variation Block.
Syntax
.DCSENS Output_Variable [File=string] [Perturbation=x]
+ [Interval=SweepValue] [Threshold=x] [GroupByDevice=0|1]
Argument
Description
Output_Variable
Response with regard to the parameters designated in Sensitivity
Block. Similar to the .DCMATCH command, the Output_Variable
can be node voltage or branch current in a circuit.
File=string
Valid file name for the output tables. Default=basename.ds# where
“#” is a number in the style of ds0, ds1, etc. If multiple dcsweep
commands are specified in the netlist, then sensitivity analysis
table results for each dcsweep are listed in *.ds# files. If .OPTION
OPFILE specified, sensitivity result tables on operating points are
listed in *.dp# files, otherwise, these tables are listed in the *.lis file.
Perturbation=x
Perturbations of x standard deviation are used in computing the
finite difference approximations to device derivatives. The valid
range for the parameter is 0.0001 to 1.0 with a default value of
0.05.
Interval=SweepValue This option only applies to one dimensional sweeps. The
SweepValue fields are positive integers. A summary is printed at
the first sweep point, then for each subsequent increment of
SweepValue, and then, if not already printed, at the final sweep
point. The Interval key is ignored with a warning if a sweep is not
being carried out.
The option only controls the printed summary table. The analysis
may be carried out at additional sweep values if required by other
forms of output such as Probe and Measure statements.
Threshold=x
Only devices with absolute sensitivity value above x are reported.
Results for all devices are displayed if Threshold=0 is set.
Default=10u.
GroupByDevice = 0|1 Alternate mode of generating sensitivity result tables; Default=0
78
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DCSENS
Description
Use this command to calculate the parameter sensitivity in the following
instances:
■
Global variation
■
Local variation
■
Local element variation with model type and model parameters that are
permitted for DCmatch, including subckt variation
The methodology is based on using a finite difference approximation algorithm.
DC sensitivity analysis combines the device derivatives, the DC solution, and
the adjoint variables to get the sensitivity. DC sensitivity analysis enables you to
compute sensitivity of any model parameter and many more models than
traditional HSPICE sensitivity analysis. In addition, the analysis supports
sensitivity for Probe and Measure output statements and for DC sweeps.
Note:
.DCSENS does not support spatial variation and global element
variation.
Examples
In the following example, the variable XVal is being swept in the DC command.
It takes nine values in sequence from 1K to 9K in increments of 1K. Tabular
output for the sensitivity command is only generated for the set XVal={1K, 4K,
7K, 9K}.
.DC XVal Start=1K Stop=9K Step=1K
.DCsens V(vcc) Interval=3
See Also
.OPTION OPFILE
DC Sensitivity Analysis and Variation Block
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
79
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DCVOLT
.DCVOLT
Sets initial conditions in HSPICE.
Syntax
.DCVOLT V(node1)=val1 V(node2)=val2 ...
.DCVOLT V node1val1 [node2val2 ...]
Argument
Description
val1 ...
Voltages. The significance of these voltages depends on whether you
specify the UIC parameter in the .TRAN command.
node1 ...
Node numbers or names can include full paths or circuit numbers.
Description
Use the .IC command or the .DCVOLT command to set transient initial
conditions in HSPICE. How it initializes depends on whether the .TRAN
analysis command includes the UIC parameter.
If you specify the UIC parameter in the .TRAN command, HSPICE does not
calculate the initial DC operating point but directly enters transient analysis.
Transient analysis uses the .IC initialization values as part of the solution for
timepoint zero (calculating the zero timepoint applies a fixed equivalent voltage
source). The .IC command is equivalent to specifying the IC parameter on
each element command but is more convenient. You can still specify the IC
parameter, but it does not take precedence over values set in the .IC
command.
If you do not specify the UIC parameter in the .TRAN command, HSPICE
computes the DC operating point solution before the transient analysis. The
node voltages that you specify in the .IC command are fixed to determine the
DC operating point. Transient analysis releases the initialized nodes to
calculate the second and later time points.
Examples
.DCVOLT 11 5 4 -5 2 2.2
See Also
.IC
.TRAN
80
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DEL LIB
.DEL LIB
Removes library data from memory for HSPICE/HSPICE RF.
Syntax
.DEL LIB ‘[file_path]file_name’ entry_name
.DEL LIB libnumberentryname
Argument
Description
entry_name
Name of entry used in the library call command to delete.
filen_ame
Name of a file to delete from the data file; the file path, plus the file
name, can be up to 256 characters long. You can use any file name that
is valid for the operating system that you use. Enclose the file path and
file name in single or double quotation marks.
file_path
Path name of a file if the operating system supports tree-structured
directories.
libnumber
Library number, used in the library call command to delete.
Description
Use this command to remove library data from memory. The next time you run
a simulation, the .DEL LIB command removes the .LIB call command with
the same library number and entry name from memory. You can then use
a .LIB command to replace the deleted library. In this way, .DEL LIB helps
you avoid name conflicts.
You can use the .DEL LIB command with the .ALTER command.
Examples
Example 1
Example 1 calculates a DC transfer function for a CMOS inverter using these
steps:
1. HSPICE simulates the device by using the NORMAL inverter model from the
MOS.LIB library.
2. Using the .ALTER block and the .LIB command, HSPICE substitutes a
faster CMOS inverter, FAST for NORMAL.
3. HSPICE then resimulates the circuit.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
81
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DEL LIB
4. Using the second .ALTER block, HSPICE executes DC transfer analysis
simulations at three different temperatures and with an n-channel width of
100 mm, instead of 15 mm.
5. HSPICE also runs a transient analysis in the second .ALTER block and
uses a .MEASURE command to measure the rise time of the inverter.
FILE1: ALTER1 TEST CMOS INVERTER
.OPTION ACCT LIST
.TEMP 125
.PARAM WVAL=15U VDD=5
*
.OP
.DC VIN 0 5 0.1
.PRINT DC V(3) V(2)
*
VDD 1 0 VDD
VIN 2 0
*
M1 3 2 1 1 P 6U 15U
M2 3 2 0 0 N 6U W=WVAL
*
.LIB 'MOS.LIB' NORMAL
.ALTER
.DEL LIB 'MOS.LIB' NORMAL $removes LIB from memory
.DEL LIB 'MOS.LIB' NORMAL $removes normal library from memory
.OPTION BRIEF=1
$suppress printing of details
.LIB 'MOS.LIB' FAST
$get fast model library
.OPTION BRIEF=0
$resume normal printing
.ALTER
.OPTION NOMOD OPTS
$suppress printing model
$parameters and print the
$option summary
.TEMP -50 0 50
$run with different temperatures
.PARAM WVAL=100U VDD=5.5 $change the parameters using
VDD 1 0 5.5
$VDD 1 0 5.5 to change the power
$supply VDD value doesn't work
VIN 2 0 PWL 0NS 0 2NS 5 4NS 0 5NS 5
$change the input source
.OP VOL
$node voltage table of
$operating points
.TRAN 1NS 5NS
$run with transient also
M2 3 2 0 0 N 6U WVAL
$change channel width
.MEAS SW2 TRIG V(3) VAL=2.5 RISE=1 TARG V(3)
+ VAL=VDD CROSS=2
$measure output
*
.END
82
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DEL LIB
Example 2
The .ALTER block adds a resistor and capacitor network to the circuit.
The network connects to the output of the inverter and HSPICE simulates
a DC small-signal transfer function.
FILE2: ALTER2.SP CMOS INVERTER USING SUBCIRCUIT
.OPTION LIST ACCT
.MACRO INV 1 2 3
M1 3 2 1 1 P 6U 15U
M2 3 2 0 0 N 6U 8U
.LIB 'MOS.LIB' NORMAL
.EOM INV
XINV 1 2 3 INV
VDD 1 0 5
VIN 2 0
.DC VIN 0 5 0. 1
.PRINT V(3) V(2)
.ALTER
.DEL LIB 'MOS.LIB' NORMAL
.TF V(3) VIN
$DC small-signal transfer
$function
*
.MACRO INV 1 2 3
$change data within
$subcircuit def
M1 4 2 1 1 P 100U 100U
$change channel length,width,also
$topology
M2 4 2 0 0 N 6U 8U
$change topology
R4 4 3 100
$add the new element
C3 3 0 10P
$add the new element
.LIB 'MOS.LIB' SLOW
$set slow model library
$.INC 'MOS2.DAT'
$not allowed to be used
$inside subcircuit, allowed
$outside subcircuit
.EOM INV
.END
See Also
.ALTER
.LIB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
83
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DESIGN_EXPLORATION
.DESIGN_EXPLORATION
Creates an Exploration Block to extract the parameters suitable for exploration
from a netlist.
Syntax
.Design_Exploration
Options
Parameter Parameter_Name = value
Parameter Parameter_Name = expression
.Data BlockName
Index Name Name, …
…
.EndData
.End_Design_Exploration
Argument Option
Description
Option Explore_only Subckts=
SubcktList
This command is executed hierarchically—the
specified subcircuits and all instantiated subcircuits
and elements underneath are affected. Thus, if an
inverter with name INV1 is placed in a digital control
block called DIGITAL and in an analog block ANALOG,
and Option Explore_only Subckts = ANALOG,
then the perturbations only affect the INV1 in the
analog block. You must create a new inverter
INV1analog, with the new device sizes.
Option Do_not_explore Subckts= Excludes listed subcircuits.
SubcktList
Option Export=yes
Exports extraction data and runs one simulation with
the original netlist
Option Export=no
(Default) Runs a simulation with Exploration data
Option Exploration_method=
external Block_name=
Block_name
The Block_name is the same as the name specified in
the .DATA block; HSPICE will sweep the row content
with the EXCommand (see Executing Exploration in
HSPICE).
Option Ignore_exploration=
yes|no
(Default=no) HSPICE ignores the content in the
design_exploration block, when
Ignore_exploration=yes.
84
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DESIGN_EXPLORATION
Argument Option
Description
Option Secondary_param= yes|no (Default = no) If Secondary_param= yes, HSPICE
exports the MOSFET secondary instance parameters
to a *.mex file (created when option export=yes),
and also permits the secondary parameters to be
imported as a column header in the .DATA block
(option export=no).
Description
Use the command to create an exploration block to extract prearrangers from a
netlist to explore in the early stages of designing integrated circuits in CMOS
technology.
Exploration is currently supported for:
■
Independent sources: DC value
■
MOS devices: W, L, M, dtemp
■
Resistors: R or W, L, M, dtemp
■
Capacitors: C or W, L, M, dtemp
When designing circuits, the multiplicity factor M is always a positive integer, but
the Exploration tool can request arbitrary positive values.
To preserve relationships which have been previously defined through
expressions, exploration can only be applied to parameters which are defined
with numerical values.
The Export and non-export modes of exploration are distinguished by setting
Export either yes or no.
The perturbation types are selected by setting any of the last three option listed
in the Argument section.
For a detailed description of the Exploration Block usage, see Exploration Block
in the HSPICE User Guide: Simulation and Analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
85
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DISTO
.DISTO
Computes the distortion characteristics of the circuit in an AC analysis.
Syntax
.DISTO Rload [inter [skw2 [refpwr spwf]]]
Argument
Description
Rload
Resistor element name of the output load resistor into which the output
power feeds.
inter
Interval at which HSPICE prints a distortion-measure summary.
Specifies a number of frequency points in the AC sweep (see the np
parameter in the .AC command).
■
If you omit inter or set it to zero, HSPICE does not print a summary.
To print or plot the distortion measures, use the .PRINT command.
■
If you set inter to 1 or higher, HSPICE prints a summary of the first
frequency and of each subsequent inter-frequency increment.
To obtain a summary printout for only the first and last frequencies, set
inter equal to the total number of increments needed to reach fstop in
the .AC command. For a summary printout of only the first frequency,
set inter to greater than the total number of increments required to
reach fstop.
HSPICE prints an extensive summary from the distortion analysis for
each frequency listed. Use the inter parameter in the .DISTO
command to limit the amount of output generated.
skw2
Ratio of the second frequency (F2) to the nominal analysis frequency
(F1) in the range 1e-3 < skw2 < 0.999. If you omit skw2, the default
value is 0.9.
refpwr
Reference power level—used to compute the distortion products. If you
omit refpwr, the default value is 1mW—measured in decibels
magnitude (dbM). The value must be ≥ 1e-10.
spwf
Amplitude of the second frequency (F2). The value must be ≥ 1e-3. The
default is 1.0.
Description
Use the .DISTO command to calculate the distortion characteristics of the
circuit in an AC small-signal, sinusoidal, steady-state analysis. The program
86
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DISTO
computes and reports five distortion measures at the specified load resistor.
The analysis assumes that the input uses one or two signal frequencies.
■
HSPICE uses the first frequency (F1, the nominal analysis frequency) to
calculate harmonic distortion. The .AC command frequency-sweep sets it.
■
HSPICE uses the optional second input frequency (F2) to calculate
intermodulation distortion. To set it implicitly, specify the skw2 parameter,
which is the F2/F1 ratio
HSPICE performs only one distortion analysis per simulation. If your design
contains more than one .DISTO command, HSPICE runs only the last
command. The .DISTO command calculates distortions for diodes, BJTs
(levels 1, 2, 3, and 4), and MOSFETs (Level49 and Level53, Version 3.22). You
can use the .DISTO command only with the .AC command.
Examples
.DISTO RL 2 0.95 1.0E-3 0.75
See Also
.AC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
87
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DOUT
.DOUT
Specifies the expected final state of an output signal.
Syntax
.DOUT nd VTH (time state [time state])
.DOUT nd VLO VHI (time state [timestate])
Argument
Description
nd
Node name
time
Absolute time point (maximum 60)
state
Expected condition of the nd node at the specified time:
■
■
■
0: Expect ZERO,LOW.
1: Expect ONE,HIGH.
Else: Do not care.
VTH
Single voltage threshold
VLO
Voltage of the logic-low state
VHI
Voltage of the logic-high state
Description
Use .DOUT to specify the expected final state of an output signal. During
simulation, HSPICE compares simulation results with the expected output. If
the states are different, an error report results.
For both syntax cases, the time, state pair describes the expected output.
During simulation, the simulated results are compared against the expected
output vector.
.DOUT State values are 0, 1, X, x, U, u, Z, z. Legal values for state are:
88
■
0: Expect zero
■
1: Expect one
■
X, x: Do not care
■
U, u: Do not care
■
Z, z: Expect high impedance (do not care)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.DOUT
In addition, HSPICE supports multiple nodes in the .DOUT statement. This
enables you to verify signals at the same time point in a single.DOUT
statement.
Examples
Example 1
The .PARAM command in this example sets the VTH variable value to 3.
The .DOUT command, operating on the node1 node, uses VTH as its
threshold voltage.
When node1 is above 3V, it is a logic 1; otherwise, it is a logic 0.
At 0ns, the expected state of node1 is logic-low.
At 2ns, 3ns, and 4ns, the expected state is “do not care.”
At 5ns, the expected state is again logic low.
.PARAM VTH=3.0
.DOUT node1 VTH(0.0n 0 1.0n 1
+ 2.0n X 3.0n U 4.0n Z 5.0n 0)
Example 2
Multiple nodes: verifying signals at the same time point
.DOUT B C D (0n 1 1 0 5n 0 0 0)
See Also
.MEASURE (or) .MEAS
.PARAM (or) .PARAMETER (or) .PARAMETERS
.PRINT
.PROBE
.STIM
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
89
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.EBD
.EBD
Invokes IBIS Electronic Board Description (EBD) functionality.
Syntax
.EBD ebdname
+ file = ’filename’
+ component = ’compname:reference_designator’
+ {component = ’compname:reference_designator’...}
+ {usemap = package_value}
Argument
Description
compname
Name after the .IBIS command that describes a component.
reference_designator Reference designator that maps the component.
package_value
Value=0,1, 2,or 3 sets the package value (the same as option
'package' of .IBIS) of all components in [Reference
Designator Map]. Default=0.
Description
Enter the .EBD command to use the IBIS EBD feature. HSPICE uses the EBD
file when simulating the line connected with the reference_designator. When
the keyword 'usemap' is added to the .EDB command, new components are
added into the circuit according to the [Reference Designator Map]. The new
component names are: 'Comp'+referenceName+'_'+ebdName
In Figure 7, CompU22_ebd and CompU23_ebd are added if U22 and U23
occur in [Reference Designator Map].
J25
Len=0.5
Len=0.5
Pin1
U21
Figure 7
Len=0.5
Pin2
U22
Pin3
U23
Circuit Connection for EBD Example
If a component is associated with both the keywords component and usemap,
then the mapping relation defined by component only is used. The format of
the node name on the EBD side is ebdName_pinName. For example, the name
J25 is ebd_J25
90
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.EBD
Note:
If a component pin is not found and it is not a terminal node in the
EBD path, then the name is used to designate the related node.
For example, in Figure 7 on page 90, if U22_2 (here, 2 is the pin
name) does not exist, then the node name will be ebd_U22_2.
If the component pin is a terminal node in the EBD path and is
not found, then the node and the associated section will not be
added into circuit. For example, in Figure 7, if U23_3 does not
exist, then the section between Pin2 and Pin3 will be ignored and
U22_2 is the terminal node.
Examples
.ebd ebd
+ file = ’test.ebd’
+ model = ’16Meg X 8 SIMM Module’
+ component = ’cmpnt:u21’
* + usemap = 0
.ibis cmpnt
+ file = ’ebd.ibs’
+ component = ’SIMM’
+ hsp_ver=2003.09 nowarn
This example corresponds to the following .ebd file:
...................
[Begin Board Description] 16Meg X 8 SIMM Module
..................
[Pin List] signal_name
J25 POWER5
[Path Description] CAS_2
Pin J25
Len=0.5 L=8.35n C=3.34p R=0.01 /
Node u21.1
Len=0.5 L=8.35n C=3.34p R=0.01 /
Node u22.2
Len=0.5 L=8.35n C=3.34p R=0.01 /
Node u23.3
See Also
.IBIS
.PKG
IBIS Examples and see .EBD command use in ebd.sp and pinmap.sp
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
91
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ELSE
.ELSE
Precedes commands to be executed in a conditional block when preceding .IF
and .ELSEIF conditions are false.
Syntax
.ELSE
Description
Use this command to precede one or more commands in a conditional block
after the last .ELSEIF command, but before the .ENDIF command.
HSPICE/HSPICE RF executes these commands by default if the conditions are
all false in the preceding .IF command and in all of the preceding .ELSEIF
commands in the same conditional block.
For the syntax and a description of how to use the .ELSE command within the
context of a conditional block, see the .IF command.
For information on use of conditional blocks with the Exploration Block, see,
Specifying Constraints in the HSPICE User Guide: Simulation and Analysis.
See Also
.ELSEIF
.ENDIF
.IF
92
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ELSEIF
.ELSEIF
Specifies conditions that determine whether HSPICE/HSPICE RF executes
subsequent commands in a conditional block.
Syntax
.ELSEIF (condition)
Description
HSPICE executes the commands that follow the first.ELSEIF command only if
condition1 in the preceding .IF command is false and condition2 in the
first .ELSEIF command is true.
If condition1 in the .IF command and condition2 in the first .ELSEIF
command are both false, then HSPICE moves on to the next .ELSEIF
command if there is one.
If this second .ELSEIF condition is true, HSPICE executes the commands that
follow the second .ELSEIF command, instead of the commands after the
first .ELSEIF command.
HSPICE ignores the commands in all false .IF and .ELSEIF commands, until
it reaches the first .ELSEIF condition that is true. If no .IF or .ELSEIF
condition is true, HSPICE continues to the .ELSE command.
For the syntax and a description of how to use the .ELSEIF command within
the context of a conditional block, see the .IF command.
For information on use of conditional blocks with the Exploration Block, see,
Specifying Constraints in the HSPICE User Guide: Simulation and Analysis.
See Also
.ELSE
.ENDIF
.IF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
93
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.END
.END
Ends a simulation run in an input netlist file.
Syntax
.END [comment]
Argument
Description
comment
Can be any comment. Typically, the comment is the name of the netlist
file or of the simulation run that this command terminates.
Description
An .END command must be the last command in the input netlist file. The
period preceding END is required. Text that follows the .END command is
regarded as a comment only. An input file that contains more than one
simulation run must include an .END command for each simulation run. You
can concatenate several simulations into a single file.
Examples
MOS OUTPUT
.OPTION NODE NOPAGE
VDS 3 0
VGS 2 0
M1 1 2 0 0 MOD1 L=4U W=6U AD=10P AS=10P
.MODEL MOD1 NMOS VTO=-2 NSUB=1.0E15 TOX=1000
+ UO=550
VIDS 3 1
.DC VDS 0 10 0.5 VGS 0 5 1
.PRINT DC I(M1) V(2)
.END MOS OUTPUT
MOS CAPS
.OPTION SCALE=1U SCALM=1U WL ACCT
.OP
.TRAN .1 6
V1 1 0 PWL 0 -1.5V 6 4.5V
V2 2 0 1.5VOLTS
MODN1 2 1 0 0 M 10 3
.MODEL M NMOS VTO=1 NSUB=1E15 TOX=1000
+ UO=800 LEVEL=1 CAPOP=2
.PRINT TRAN V(1) (0,5) LX18(M1) LX19(M1) LX20(M1)
+ (0,6E-13)
.END MOS CAPS
94
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENDDATA
.ENDDATA
Ends a .DATA block in an HSPICE input netlist file.
Syntax
.ENDDATA
Description
Use this command to terminate a .DATA block in an HSPICE input netlist.
See Also
.DATA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
95
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENDIF
.ENDIF
Ends a conditional block of commands in an HSPICE input netlist file.
Syntax
.ENDIF
Description
Use this command to terminate a conditional block of commands that begins
with an .IF command.
For the syntax and a description of how to use the .ENDIF command within the
context of a conditional block, see the .IF command.
See Also
.ELSE
.ELSEIF
.IF
96
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENDL (or) .ENDL TT
.ENDL (or) .ENDL TT
Ends a .LIB command in an HSPICE/HSPICE RF input netlist file.
Syntax
.ENDL
.ENDL TT
Description
Use this command to terminate a .LIB command in an HSPICE input netlist.
Examples
Either the .ENDL or .ENDL TT command is valid for ending a .LIB statement.
.lib tt
.param vth=0.1
.include 'model_tt.sp'
.endl tt
or
.lib tt
.param vth=0.1
.include 'model_tt.sp'
.endl
See Also
.LIB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
97
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENDS
.ENDS
Ends a subcircuit definition (.SUBCKT) in an HSPICE input netlist file.
Syntax
.ENDS subckt_name
Argument
Description
subckt_name
Subcircuit name definition to end a command that begins with
a .SUBCKT command.
Description
Use this command to terminate a .SUBCKT command. This command must be
the last for any subcircuit definition that starts with a .SUBCKT command. You
can nest subcircuit references (calls) within subcircuits in HSPICE.
Note:
Using -top subck_name on the command line effectively
eliminates the need for the .subckt subckt_name and
.ends subckt_name
Examples
Example 1
Terminates a subcircuit named mos_circuit.
.ENDS mos_circuit
Example 2
Terminates all subcircuit definitions that begin with a .SUBCKT
command.
.ENDS
See Also
.SUBCKT
98
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENV
.ENV
Performs standard envelope simulation in HSPICE RF.
Syntax
.ENV TONES=f1 [f2...fn] NHARMS=h1[h2...hn]
+ ENV_STEP=tstep ENV_STOP=tstop
Argument
Description
TONES
Carrier frequencies, in hertz
NHARMS
Number of harmonics
ENV_STEP
Envelope step size, in seconds
ENV_STOP
Envelope stop time, in seconds
Description
Use this command to perform standard envelope simulation.
The simulation proceeds just as it does in standard transient simulation,
starting at time=0 and continuing until time=env_stop. An HB analysis is
performed at each step in time. You can use Backward-Euler (BE), trapezoidal
(TRAP), or level-2 Gear (GEAR) integration.
■
For BE integration, set .OPTION SIM_ORDER=1.
■
For TRAP, set .OPTION SIM_ORDER=2 (default) METHOD=TRAP (default).
■
For GEAR, set .OPTION SIM_ORDER=2 (default) METHOD=GEAR.
See Also
.ENVOSC
.HB
.PRINT
.PROBE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
99
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENVFFT
.ENVFFT
Performs Fast Fourier Transform (FFT) on envelope output in HSPICE RF.
Syntax
.ENVFFT output_var NP=value FORMAT=keyword
+ WINDOW=keyword ALFA=value
Argument
Description
output_var
Any valid output variable.
NP
Number of points to use in the FFT analysis. NP must be a power
of 2. If not a power of 2, then it is automatically adjusted to the
closest higher number that is a power of 2. The default is 1024.
FORMAT
Output format:
NORM= normalized magnitude
UNORM=unnormalized magnitude (default)
WINDOW
Window type to use:
■
■
■
■
■
■
■
■
ALFA
RECT=simple rectangular truncation window (default)
BART=Bartlett (triangular) window
HANN=Hanning window
HAMM=Hamming window
BLACK=Blackman window
HARRIS=Blackman-Harris window
GAUSS=Gaussian window
KAISER=Kaiser-Bessel window
Controls the highest side-lobe level and bandwidth for GAUSS and
KAISER windows. The default is 3.0.
Description
Use this command to perform Fast Fourier Transform (FFT) on envelope
output. This command is similar to the .FFT command. In HSPICE RF the data
being transformed is complex. You usually want to do this for a specific
harmonic of a voltage, current, or power signal.
See Also
.ENV
.ENVOSC
.FFT
100
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ENVOSC
.ENVOSC
Performs envelope simulation for oscillator startup or shutdown in HSPICE RF.
Syntax
.ENVOSC TONE=f1 NHARMS=h1 ENV_STEP=tstep ENV_STOP=tstop
+ PROBENODE=n1,n2,vosc [FSPTS=num, min, max]
Argument
Description
TONES
Carrier frequencies, in hertz.
NHARMS
Number of harmonics.
ENV_STEP
Envelope step size, in seconds.
ENV_STOP
Envelope stop time, in seconds.
PROBENODE
Defines the nodes used for oscillator conditions and the initial probe
voltage value.
FSPTS
Specifies the frequency search points used in the initial small-signal
frequency search. Usage depends on oscillator type.
Description
Use .EVOSC to perform envelope simulation for oscillator startup or shutdown.
Oscillator startup or shutdown analysis must be helped along by converting a
bias source from a DC description to a PWL description that either:
■
Starts at a low value that supports oscillation and ramps up to a final value
(startup simulation)
■
Starts at the DC value and ramps down to zero (shutdown simulation).
In addition to computing the state variables at each envelope time point, the
.ENVOSC command also computes the frequency. This command is applied to
high-Q oscillators that take a long time to reach steady-state. For these circuits,
standard transient analysis is too costly. Low-Q oscillators, such as typical ring
oscillators are more efficiently simulated with standard transient analysis.
See Also
.ENV
.ENVFFT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
101
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.EOM
.EOM
Ends a .MACRO command.
Syntax
.EOM subckt_name
ArgumentArgument
DescriptionDescription
subckt_name
Subcircuit name definition to end a macro that begins with
a .SUBCKT command.
Description
Use this command to terminate a .MACRO command..EOM must be the last for
any subcircuit definition that starts with a .MACRO command. You can nest
subcircuit references (calls) within subcircuits.
Examples
Example 1
Terminates a subcircuit named diode_circuit.
.EOM diode_circuit
Example 2
If you omit the subcircuit name as in this second example, this command
terminates all subcircuit definitions that begin with a .MACRO command.
.EOM
See Also
.MACRO
102
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FFT
.FFT
Calculates the Discrete Fourier Transform (DFT) value used for spectrum
analysis. Numerical parameters (excluding string parameters) can be passed
to the .FFT command.
Syntax
Syntax # 1 Alphanumeric input
.FFT output_var [START=value] [STOP=value]
+ NP=value [FORMAT=keyword
+ [WINDOW=keyword] [ALFA=value]
+ [FREQ=value [FMIN=value] [FMAX=value]
Syntax #2 Numerics and expressions
.FFT [output_var] [START=param_expr1] [STOP=param_expr2]
+ [NP=param_expr3] [FORMAT=keyword]
+ [WINDOW=keyword] [ALFA=param_expr4]
+ [FREQ=param_expr5] [FMIN=param_expr6] [FMAX=param_expr7]
Syntax # Verilog-A Blocks
.FFT VAblock:SigName StartIdx=n1 StartIdx=n2
+ SamplePeriod=val
+ ...
Argument
Description
output_var
Any valid output variable, such as voltage, current, or power.
START
Start of the output variable waveform to analyze. Defaults to the START value
in the .TRAN command (tstart), which defaults to 0.
FROM
An alias for START in .FFT commands.
STOP
End of the output variable waveform to analyze. Defaults to the TSTOP value
in the .TRAN command.
TO
An alias for STOP, in .FFT commands.
NP
Number of points to use in the FFT analysis. NP must be a power of 2. If NP
is not a power of 2, HSPICE automatically adjusts it to the closest higher
number that is a power of 2. The default is 1024.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
103
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FFT
Argument
Description
FORMAT
Output format:
■
■
WINDOW
NORM= normalized magnitude (default)
UNORM=unnormalized magnitude
Window can be one of the following types:
■
■
■
■
■
■
■
■
RECT=simple rectangular truncation window (default).
BART=Bartlett (triangular) window.
HANN=Hanning window.
HAMM=Hamming window.
BLACK=Blackman window.
HARRIS=Blackman-Harris window.
GAUSS=Gaussian window.
KAISER=Kaiser-Bessel window.
ALFA
Parameter to use in GAUSS and KAISER windows to control the highest sidelobe level, bandwidth, and so on.
1.0 <= ALFA <= 20.0
The default is 3.0
FREQ
Frequency to analyze. If FREQ is non-zero, the output lists only the harmonics
of this frequency, based on FMIN and FMAX. HSPICE also prints the THD for
these harmonics. The default is 1.0 (STOP-START) (Hz).
FMIN
Minimum frequency for which HSPICE prints FFT output into the listing file.
THD calculations also use this frequency.
T=(STOP-START)
The default is 1.0/T (Hz).
FMAX
Maximum frequency for which HSPICE prints FFT output into the listing file.
THD calculations also use this frequency. The default is 0.5*NP*FM IN (Hz).
VAblock
Name of the Verilog-A block.
SigName
Parameter name of the series output from Verilog-A. It should have the
following type definition in Verilog-A block:
(* desc="SigName" *) real SigName[n1:n2];
StartIdx
Start index of the series for FFT.
StopIdx
End index of the series for FFT; it must be greater than StartIdx; otherwise,
HSPICE uses the whole series for the FFT process.
104
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FFT
Argument
Description
SamplePeriod
Time interval between two samples inside the series. It must be a positive
value, the default value is 1 second.
Description
Use this command to calculate the Discrete Fourier Transform (DFT) values for
spectrum analysis. .FFT uses internal time point values to calculate these
values. A DFT uses sequences of time values to determine the frequency
content of analog signals in circuit simulation. You can pass numerical
parameters/expressions (but no string parameters) to the .FFT command.
Output variables for .FFT can be voltage, current, or power, followed by a
parenthesis containing the instance name. If it is power, for example, you need
to write the signal’s name in the format p(instance_name).
You can specify only one output variable in an .FFT command. The following is
an incorrect use of the command because it contains two variables in
one .FFT command:
For an .FFT analysis using a Verilog A-block, the FFT time window is:
TimeWindow = SamplePeriod*(stopidx-startidx)
A FFT process requires sampling the waveform with equally spaced time
points, and the total point number must be 2N (N: integer). Therefore, the start/
stop time points, fundamental frequency, sampling rate, and total point number
are not independent of each other. They need to satisfy the following
relationship:
point_number
------------------------------------ = sample rate, where point_number = 2 N
t stop – t start
M
F fund = ---------------------------, where M is an integer number
t stop – t start
If that relationship is compromised, conflicts between parameters may arise. To
avoid such conflicts, HSPICE conducts an error check process according to the
following:
Parameter
Check if input...
Adjust if input...
Set if not input...
START
Error if < tstart (start point in
.TRAN)
N/A
=tstart (start point in
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
105
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FFT
Parameter
Check if input...
Adjust if input...
Set if not input...
STOP
Error if > tstop (stop point in
.TRAN)
N/A
=tstop (stop point in
.TRAN
NP
Error if NP< 4Error if NP > 227 Is not a power of 2;
adjust to nearest
power of 2, issue
warning and final
value
FREQ
1
STOP – START
Error if < ---------------------------------------
SamplePeriod Error if non-positive
Default value (1024)
If not integer multiple
of 1/(STOP-START)),
adjust to nearest
multiple of
1/(STOP-START),
issue warning and
final value
1
-------------------------------------STOP – START
Use default value: 1s
1 second
StartIdx
Error if ≥ StopIdx
N/A
Start index of the VA
array
StopIdx
Error if ≤ StartIdx
N/A
Stop index of the VA
array
An embedded .FFT command in a measure_file can be called to perform FFT
measurements from previous simulation results as follows:
HSPICE -i *.tr0 -meas measure_file
Examples
.FFT v(1)
.FFT v(1,2) np=1024 start=0.3m stop=0.5m freq=5.0k
+ window=kaiser alfa=2.5
.FFT I(rload) start=0m to=2.0m fmin=100k fmax=120k
+ format=unorm
.FFT par(‘v(1) + v(2)’) from=0.2u stop=1.2u
+ window=harris
The example below generates an .ft0 file for the FFT of v(1) and an .ft1 file for
the FFT of v(2).
.FFT v(1) np=1024
.FFT v(2) np=1024
106
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FFT
See Also
.TRAN
.MEASURE FFT
Spectrum Analysis
Fourier Analysis Examples for demo files on window weighting including
• gauss.sp
•
hamm.sp
•
hann.sp
•
harris.sp
•
kaiser.sp
•
rect.sp
Fourier Analysis Examples, netlists demonstrating use of the .FFT
command:
• fft5.sp (data-driven with transient analysis)
•
fft6.sp and sine.sp (sine source)
•
intermod.sp (intermodulation distortion)
•
mod.sp (modulated pulse)
•
pulse.sp (pulse source)
•
pwl.sp (PWL source)
•
sffm.sp (single-frequency FM source)
•
swcap5.sp (fifth-order elliptic, switched-capacitor filter)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
107
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FLAT
.FLAT
Provides subcircuit OP back annotation when a device is modeled as a subckt.
Syntax
If defined in subckt definition block:
.FLAT element_name
If defined in main circuit:
.FLAT subckt_nameelement_name
Description
This command enables subcircuit OP back annotation when a device is
modeled as a subckt.
Note:
subckt_name is the name appearing in a .subckt definition
statement; element_name is a simple element name which is
defined in the same subckt definition block.
When a device is modeled as a subcircuit rather than as .MODEL, using the
.FLAT command within a subcircuit allows the writing of a results file with
proper values for the device. Back-annotation is done by retrieving results from
the input.op0 (for DC) and input.op1 (for transient) results files. The .FLAT
command works for *.wdf format, *.psf, and *.tr0 files.
This subckt file
...is equal to
.subckt nmos_sub d g s b
m0 d g s b nmos 10u 10u
r0 int_d d 100
.flat m0
.model nmos nmos level=49
.ends nmos_sub
.flat nmos_sub m0
.subckt nmos_sub d g s b
m0 d g s b nmos 10u 10u
r0 int_d d 100
.model nmos nmos level=49
.ends nmos_sub
If the .FLAT command is in both the subckt definition block and main circuit,
the subckt block .FLAT takes priority. If more than one .FLAT is defined for the
same subckt, the last one takes priority.
108
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FLAT
Examples
.subckt nmossub D G S B l=l w=w
M1 D_int G_int S_int B nch l=l w=w
M2 D_int G_int S_int B nch l=l w=w
RD D D_int 100
RG G G_int 10
RS S S_int 400
.flat M1
.ends nmossub
X1 1 2 0 0 nmossub
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
109
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FOUR
.FOUR
Performs a Fourier analysis as part of the transient analysis.
Syntax
.FOUR freq ov1 [ov2 ov3 ...]
Argument
Description
freq
Fundamental frequency
ov1 ...
Output variables to analyze
Description
Use this command to perform a Fourier analysis as part of the transient
analysis. You can use this command in HSPICE to perform the Fourier analysis
over the interval (tstop-fperiod, tstop), where:
■
tstop is the final time, specified for the transient analysis.
■
fperiod is a fundamental frequency period (freq parameter).
HSPICE performs Fourier analysis on 501 points of transient analysis data on
the last 1/f time period, where f is the fundamental Fourier frequency. HSPICE
interpolates transient data to fit on 501 points, running from (tstop-1/f) to tstop.
To calculate the phase, the normalized component and the Fourier component,
HSPICE uses 10 frequency bins. The Fourier analysis determines the DC
component and the first nine AC components. For improved accuracy,
the .FOUR command can use non-linear, instead of linear interpolation.
You can use a .FOUR command only with a .TRAN command.
Examples
.FOUR 100K V(5)
See Also
.TRAN
.FFT
110
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FSOPTIONS
.FSOPTIONS
Sets various options for the HSPICE Field Solver.
Syntax
.FSOPTIONS name [ACCURACY=LOW|MEDIUM|HIGH]
+ [GRIDFACTOR=val] [PRINTDATA=YES|NO]
+ [COMPUTE_GO=YES|NO] [COMPUTE_GD=YES|NO]
+ [COMPUTE_RO=YES|NO] [COMPUTE_RS=YES|NO]
+ [COMPUTE_RS=YES|NO|DIRECT|ITER]
+ [COMPUTE_TABLE=FREQENCY_SWEEP]
+ [PRINTDATA=YES|NO|APPEND]
Argument
Description
name
Option name.
ACCURACY
Solver accuracy is one of the following:
■
■
■
GRIDFACTOR
LOW
MEDIUM
HIGH
Multiplication factor (integer) to determine the final number of
segments used to define the shape.
If you set COMPUTE_RS=yes, the field solver does not use this
parameter to compute Ro and Rs values.
PRINTDATA
Prints output matrixes to a file.
COMPUTE_GO
Computes the static conductance matrix.
COMPUTE_GD
Computes the dielectric loss matrix.
COMPUTE_RO
Computes the DC resistance matrix.
COMPUTE_RS
Activates and chooses filament solver to compute Ro and Rs. The
solver computes the skin-effect resistance matrix.
■
■
■
■
YES: activate filament solver with direct matrix solver
NO: (Default) Does not perform filament solver
DIRECT: Activate filament solver with direct matrix solver
(same as “YES”)
ITER: Activates filament solver with iterative matrix solver
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
111
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FSOPTIONS
Argument
Description
COMPUTE_TABLE Specifies a type of frequency sweep for extracting RLGC Tabular
Model. You can specify either LIN, DEC, OCT, POI. Specify the
nsteps, start, and stop values using the following syntax for each
type of sweep:
■
■
■
■
PRINTDATA
LIN
DEC
OCT
POI
nsteps
nsteps
nsteps
nsteps
start stop
start stop
start stop
freq_values
When PRINTDATA=APPEND, RLGC model output is appended
to the specified output file.
Description
Use the .FSOPTIONS command to set various options for the field solver. The
following rules apply to the field solver when specifying options with
the .FSOPTIONS command:
■
The field solver always computes the L and C matrixes.
■
If COMPUTE_RS=YES, the field solver starts and calculates Lo, Ro, and Rs.
■
For each accuracy mode, the field solver uses either the predefined number
of segments or the number of segments that you specified. It then multiplies
this number times the GRIDFACTOR to obtain the final number of segments.
Because a wide range of applications are available, the predefined accuracy
level might not be accurate enough for some applications. If you need a higher
accuracy than the value that the HIGH option sets, then increase either the
GRIDFACTOR value or the N, NH, or NW values to increase the mesh density. NW
and NH quantities are used for rectangles and N is used for circles, polygons
and strips. See the .SHAPE commands in this chapter for the complete syntax
for each shape.
Note:
The forms of the following arguments are interchangeable:
COMPUTE_GO : COMPUTEGO
COMPUTE_GD : COMPUTEGD
COMPUTE_RO : COMPUTERO
COMPUTE_RS : COMPUTERS
COMPUTE_TABLE : COMPUTETABLE
See the HSPICE User Guide: Signal Integrity for more information on
Extracting Transmission Line Parameters (Field Solver).
112
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.FSOPTIONS
Examples
// LU solver
*.fsoptions printem printdata=yes compute_rs=direct
compute_gd=yes
// GMRES solver
.fsoptions printem printdata=yes compute_rs=iter compute_gd=yes
See Also
.LAYERSTACK
.MATERIAL
.SHAPE
Transmission (W-element) Line Examples
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
113
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.GLOBAL
.GLOBAL
Globally assigns a node name.
Syntax
.GLOBAL node1 node2 node3 ...
Argument
Description
node1, node2...
Name of a global nodes, such as supply and clock names; overrides
local subcircuit definitions.
Description
Use this command to globally assign a node name in HSPICE. This means that
all references to a global node name, used at any level of the hierarchy in the
circuit, connect to the same node.
The most common use of a .GLOBAL command is if your netlist file includes
subcircuits. This command assigns a common node name to subcircuit nodes.
Another common use of .GLOBAL commands is to assign power supply
connections of all subcircuits. For example, .GLOBALVCC connects all
subcircuits with the internal node name VCC.
Typically, in a subcircuit, the node name consists of the circuit number
concatenated to the node name. When you use a .GLOBAL command,
HSPICE does not concatenate the node name with the circuit number and
assigns only the global name. You can then exclude the power node name in
the subcircuit or macro call.
Examples
This example shows global definitions for VDD and input_sig nodes.
.GLOBAL VDD input_sig
114
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HB
.HB
Invokes the single and multitone harmonic balance algorithm for periodic
steady state analysis.
Syntax
Syntax # 1 without SS_TONE
.HB TONES=F1 [F2 … FN] [SUBHARMS=SH]
+ [NHARMS=H1, H2 … HN] [INTMODMAX=n]
+ [SWEEP parameter_sweep]
Syntax#2 with SS_TONE
.HB TONES=F1 [F2 … FN] [SUBHARMS=SH]
+ [NHARMS=H1, H2 … HN] [INTMODMAX=n]
+ [SS_TONE=n] [SWEEP parameter_sweep]
Argument
Description
TONES
Fundamental frequencies.
SUBHARMS
Subharmonics in the analysis spectrum. The minimum non-DC frequency in the
analysis spectrum is f/subharms, where f is the frequency of oscillation.
NHARMS
Number of harmonics to use for each tone. Must have the same number of entries
as TONES. You must specify NHARMS, INTMODMAX or both.
INTMODMAX Maximum intermodulation product order that you can specify in the analysis
spectrum. You must specify NHARMS, INTMODMAX or both.
SWEEP
Type of sweep. You can sweep up to three variables. You can specify either LIN,
DEC, OCT, POI, SWEEPBLOCK, DATA, OPTIMIZE or MONTE. Specify the
nsteps, start, and stop times using the following syntax for each type of sweep:
■
■
■
■
■
■
■
■
SS_TONE
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA=dataname
OPTIMIZE=OPTxxx
MONTE=val
Small-signal tone number for HBLIN analysis. The value must be an integer
number. The default value is 0, indicating that no small signal tone is specified.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
115
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HB
Description
Use this command to invoke the single and multitone harmonic balance
algorithm for periodic steady state analysis.
The NHARMS and INTMODMAX input parameters define the spectrum.
■
If INTMODMAX=N, the spectrum consists of all f=a*f1 + b*f2 + ... + n*fn
frequencies so that f>=0 and |a|+|b|+...+|n|<=N. The a,b,...,n coefficients are
integers with absolute value <=N.
■
If INTMODMAX is not specified, HSPICE RF defaults it to the largest value in
the NHARMS list.
■
If entries in the NHARMS list are > INTMODMAX, HSPICE RF adds the m*fk
frequencies to the spectrum, where fk is the corresponding tone, and m is a
value <= the NHARMS entry.
For detailed discussion of HBLIN analysis, see Frequency Translation SParameter (HBLIN) Extraction in the HSPICE User Guide: RF Analysis.
Examples
In Example 1, the resulting HB analysis spectrum={dc, f1, f2}.
Example 1
.hb tones=f1, f2 intmodmax=1
In Example 2, the HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2}.
Example 2
.hb tones=f1, f2 intmodmax=2
In Example 3, the resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1,
2*f2, 2*f1+f2, 2*f1-f2, 2*f2+f1, 2*f2-f1, 3*f1, 3*f2}.
Example 3
.hb tones=f1, f2 intmodmax=3
In Example 4, the resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2,
2*f1,2*f2}.
Example 4
.hb tones=f1, f2 nharms=2,2
116
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HB
In Example 5, the resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1,
2*f2, 2*f1-f2, 2*f1+f2, 2*f2-f1, 2*f2+f1}.
Example 5
hb tones=f1, f2 nharms=2,2 intmodmax=3
The resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2, 2*f1-f2,
2*f1+f2, 2*f2-f1, 2*f2+f1, 3*f1, 3*f2, 4*f1, 4*f2, 5*f1, 5*f2}.
Example 6
.hb tones=f1, f2 nharms=5,5 intmodmax=3
See Also
.ENV
.HBAC
.HBLIN
.HBNOISE
.HBOSC
.OPTION HBCONTINUE
.OPTION HBJREUSE
.OPTION HBJREUSETOL
.OPTION HBACKRYLOVDIM
.OPTION HBKRYLOVTOL
.OPTION HBLINESEARCHFAC
.OPTION HBMAXITER (or) HB_MAXITER
.OPTION HBSOLVER
.OPTION HBTOL
.OPTION LOADHB
.OPTION SAVEHB
.OPTION TRANFORHB
.PRINT
.PROBE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
117
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBAC
.HBAC
Performs harmonic-balance–based periodic AC analysis on circuits operating
in a large-signal periodic steady state.
Syntax
.HBAC frequency_sweep
Argument
Description
frequency_sweep
Frequency sweep range for the input signal (also refer to as
the input frequency band (IFB) or fin). You can specify LIN,
DEC, OCT, POI, SWEEPBLOCK, or DATA. Specify the
nsteps, start and stop times using the following syntax for
each type of sweep:
■
■
■
■
■
■
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA=dataname
Description
Use this command to invoke a harmonic balance-based periodic AC analysis to
analyze small-signal perturbations on circuits operating in a large-signal
periodic steady state.
See Also
.HB
.HBNOISE
.HBOSC
.OPTION HBACTOL
.OPTION HBACKRYLOVDIM
.PRINT
.PROBE
118
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBLIN
.HBLIN
Extracts frequency translation S-parameters and noise figures.
Syntax
Without SS_TONE
.HBLIN frequency_sweep
+ [NOISECALC=1|0|yes|no] [FILENAME=file_name]
+ [DATAFORMAT=ri|ma|db]
+ [MIXEDMODE2PORT=dd|cc|cd|dc|sd|sc|cs|ds]
With SS_TONE
.HBLIN [NOISECALC=1|0|yes|no] [FILENAME=file_name]
+ [DATAFORMAT=ri|ma|db]
+ [MIXEDMODE2PORT=dd|cc|cd|dc|sd|sc|cs|ds]
Argument
Description
frequency_sweep
Frequency sweep range for the input signal (also referred to as
the input frequency band (IFB) or fin). You can specify LIN,
DEC, OCT, POI, SWEEPBLOCK, or DATA. Specify the nsteps,
start, and stop times using the following syntax for each type of
sweep:
■
■
■
■
■
■
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA=dataname
NOISECALC
Enables calculating the noise figure. The default is no (0).
FILENAME
Output file name for the extracted S-parameters or the object
name after the -o command-line option. The default is the
netlist file name.
DATAFORMAT
Format of the output data file.
■
■
■
dataformat=RI, real-imaginary. This is the default for .sc#/citi
file.
dataformat=MA, magnitude-phase. This is the default format
for Touchstone file.
dataformat=DB, DB(magnitude)-phase.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
119
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBLIN
Argument
Description
MIXEDMODE2PORT Mixed-mode data map of output mixed mode S-parameter
matrix. The availability and default value for this keyword
depends on the first two port (P element) configuration as
follows:
■
■
■
■
case 1: p1=p2=single-ended (standard-mode P element)
available: ss
default: ss
case 2: p1=p2=balanced (mixed-mode P element)
available: dd, cd, dc, cc
default: dd
case 3: p1=balanced p2=single-ended
available: ds, cs
default: ds
case 4: p1=single p2=balanced
available: sd, sc
default: sd
Description
Use this command in HSPICE RF to extract frequency translation Sparameters and noise figures.
See Also
.HB
.HBAC
.PRINT
.PROBE
120
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBLSP
.HBLSP
Performs periodically driven nonlinear circuit analyses for power-dependent
S parameters.
Syntax
.HBLSP NHARMS=nh [POWERUNIT=dbm|watt]
+ [SSPCALC=1|0|YES|NO] [NOISECALC=1|0|YES|NO]
+ [FILENAME=file_name] [DATAFORMAT=ri|ma|db]
+ FREQSWEEP freq_sweep POWERSWEEP power_sweep
Argument
Description
NHARMS
Number of harmonics in the HB analysis triggered by the .HBLSP
command.
POWERUNIT
Power unit. Default is watt.
SSPCALC
Extract small-signal S-parameters. Default is 0 (NO).
NOISECALC
Perform small-signal 2-port noise analysis. Default is 0 (NO).
FILENAME
Output data .p2d# filename. Default is the netlist name or the object
name after the -o command-line option.
DATAFORMAT
Format of the output data file. Default is ma (magnitude, angle).
FREQSWEEP
Frequency sweep specification. A sweep of type LIN, DEC, OCT,
POI, or SWEEPBLOCK. Specify the nsteps, start, and stop times
using the following syntax for each type of sweep:
■
LIN nsteps start stop
DEC nsteps start stop
■
OCT nsteps start stop
■
POI nsteps freq_values
■
SWEEPBLOCK=blockname
This keyword must appear before the POWERSWEEP keyword.
■
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
121
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBLSP
Argument
Description
POWERSWEEP Power sweep specification. A sweep of type LIN, DEC, OCT,POI, or
SWEEPBLOCK. Specify the nsteps, start, and stop times using the
following syntax for each type of sweep:
■
LIN nsteps start stop
DEC nsteps start stop
■
OCT nsteps start stop
■
POI nsteps power_values
■
SWEEPBLOCK=blockname
This keyword must follow the FREQSWEEP keyword.
■
Description
Use this command in HSPICE RF to invoke periodically driven nonlinear circuit
analyses for power-dependent S-parameters.
For details, see the HSPICE User Guide: RF Analysis, Large-Signal Sparameter (HBLSP) Analysis.
See Also
.HB
.PRINT
.PROBE
122
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBNOISE
.HBNOISE
Performs cyclo-stationary noise analysis on circuits operating in a large-signal
periodic steady state.
Syntax
.HBNOISE [output] [insrc] [parameter_sweep]
+ [n1, n2, …, nk,+/-1]
+ [listfreq=(frequencies|none|all)] [listcount=val]
+ [listfloor=val] [listsources=on|off]
Argument
Description
output
Output node, pair of nodes, or 2-terminal element. HSPICE RF references
equivalent noise output to this node (or pair of nodes). Specify a pair of
nodes as V(n+,n-). If you specify only one node, V(n+), then HSPICE RF
assumes that the second node is ground. You can also specify a 2-terminal
element name that refers to an existing element in the netlist.
insrc
Input source. If this is a resistor, HSPICE RF uses it as a reference noise
source to determine the noise figure. If the resistance value is 0, the result
is an infinite noise figure.
parameter_sweep
Frequency sweep range for the input signal. Also referred to as the input
frequency band (IFB) or fin). You can specify LIN, DEC, OCT, POI,
SWEEPBLOCK, DATA, MONTE, or OPTIMIZE sweeps. Specify the nsteps,
start, and stop frequencies using the following syntax for each type of
sweep:
■
■
■
■
■
■
■
■
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA dataname
MONTE niterations
OPTIMIZE optxxx
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
123
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBNOISE
Argument
Description
n1,n2,...,nk, +/-1
Index term defining the output frequency band (OFB or fout) at which the
noise is evaluated. Generally, fout=ABS(n1*f+n2*f2+...+nk*fk+/-fin) Where:
■
f1,f2,...,fk are the first through k-th steady-state tones determined from
the harmonic balance solution
■
n1,n2,...,nk are the associated harmonic multipliers
■
fin is the IFB defined by parameter_sweep.
The default index term is [1,1,...1,-1]. For a single tone analysis, the default
mode is consistent with simulating a low-side, down conversion mixer where
the RF signal is specified by the IFB and the noise is measured at a downconverted frequency that the OFB specifies. In general, you can use the
[n1,n2,...,nk,+/-1] index term to specify an arbitrary offset. The noise figure
measurement is also dependent on this index term.
listfreq
Prints the element noise value to the .lis file. You can specify at which
frequencies the element noise value is printed. The frequencies must match
the sweep_frequency values defined in the parameter_sweep, otherwise
they are ignored.In the element noise output, the elements that contribute
the largest noise are printed first. The frequency values can be specified
with the NONE or ALL keyword, which either prints no frequencies or every
frequency defined in parameter_sweep. Frequency values must be
enclosed in parentheses. For example:listfreq=(none)
listfreq=(all) listfreq=(1.0G) listfreq=(1.0G, 2.0G)The
default value is NONE.
listcount
Prints the element noise value to the .lis file, which is sorted from the largest
to smallest value. You do not need to print every noise element; instead, you
can define listcount to print the number of element noise frequencies.
For example, listcount=5 means that only the top 5 noise contributors
are printed. The default value is 1.
listfloor
Prints the element noise value to the .lis file and defines a minimum
meaningful noise value (in V/Hz1/2 units). Only those elements with noise
values larger than listfloor are printed. The default value is 1.0e-14 V/
Hz1/2.
listsources
Prints the element noise value to the .lis file when the element has multiple
noise sources, such as a FET, which contains the thermal, shot, and 1/f
noise sources. You can specify either ON or OFF: ON Prints the contribution
from each noise source and OFF does not. The default value is OFF.
124
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBNOISE
Description
Use this command to invoke cyclo-stationary noise analysis on circuits
operating in a large-signal periodic steady state.
See Also
.HB
.HBAC
.HBOSC
.PRINT
.PROBE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
125
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBOSC
.HBOSC
Performs oscillator analysis on autonomous (oscillator) circuits. The input
syntax for HBOSC analysis supports two different formats, depending on
whether the PROBENODE location is specified using a circuit element (current
source) or using the HBOSC PROBENODE parameters:
Syntax
Syntax #1
.HBOSC TONE=F1 NHARMS=H1
+ PROBENODE=N1,N2,VP
+[FSPTS=NUM, MIN, MAX] [STABILITY=(-2|-1|0|1|2)]
+[SWEEP PARAMETER_SWEEP] [SUBHARMS=I]
Syntax #2 (Uses current source to set PROBENODE)
ISRC N1N2 HBOSCVPROBE=VP
.HBOSC TONE=F1 NHARMS=H1
+[FSPTS=NUM, MIN, MAX] [STABILITY=(-2|-1|0|1|2)]
+[SWEEP PARAMETER_SWEEP] [SUBHARMS=I]
Argument
Description
TONE
Approximate value for oscillation frequency (Hz). The search for an exact
oscillation frequency begins from this value unless you specify an FSPTS
range or transient initialization.
NHARMS
Number of harmonics to use for oscillator HB analysis.
PROBENODE
Circuit nodes that are probed for oscillation conditions.
■
N1 and N2 are the positive and negative nodes for a voltage probe
inserted in the circuit to search for oscillation conditions.
■
VP is the initial probe voltage value (suggested: 1/2 the supply voltage).
The phase of the probe voltage is forced to zero; all other phases are relative
to the probe phase. HSPICE RF uses this probe to calculate small-signal
admittance for the initial frequency estimates. It should be connected near
the “heart” of the oscillator (near resonators, inside the ring of a ring
oscillator, and so on). Note: The PROBENODE pins and approximate
voltage value can also be set by using a zero amp current source that uses
the HBOSCVPROBE keyword.
HBOSCVPROBE
= VP
126
Sets PROBENODE with a current source. If a current source with
HBOSCVPROBE is used, the PROBENODE syntax is not necessary.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBOSC
Argument
Description
FSPTS
Frequency search points that HSPICE RF uses in its initial small-signal
frequency search to find an oscillation frequency. Optional, but
recommended for high-Q and most LC oscillators.
■
NUM is an integer.
MIN and MAX are frequency values in units of Hz.
If the FSPTS analysis finds an approximate oscillation frequency, the TONE
parameter is ignored. An option for FSPTS
■
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
127
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBOSC
Argument
Description
STABILITY
When used with FSPTS, activates the additional oscillator stability analyses
depending on the following values:
■
■
■
■
■
128
0: A single point oscillator frequency-search stability analysis is
performed. The FSPTS search is executed, and the first successful linear
oscillation frequency value found is used as the starting point for the twotier Newton nonlinear oscillator analysis. The probenode vp value
specified is used as the starting amplitude for the Newton solver.
1: (default) A single point oscillator frequency-search stability analysis,
plus an estimate of oscillator amplitude, is performed. The FSPTS search
is executed, and the first successful linear oscillation frequency value
found is used as the starting point for the two-tier Newton nonlinear
oscillator analysis. An additional analysis for automatically estimating the
probenode amplitude is also performed, and this value is used as the
starting amplitude for the two-tier Newton solver.
–1: A single point oscillator frequency-search stability analysis, plus an
estimate of oscillator amplitude, is performed. The FSPTS search is
executed, and the first successful linear oscillation frequency value found
is accurately computed and reported. An additional analysis for
automatically estimating the probenode amplitude is also performed, and
this value is also reported. The analysis aborts without attempting the
two-tier Newton nonlinear oscillator analysis. By using STABILITY=–1, a
check can be made if any linear oscillation conditions are found, before
attempting the nonlinear oscillator analysis.
2: A multipoint frequency-search stability analysis is performed. The
FSPTS search is executed, and all successful linear oscillation frequency
values found over the entire FSPTS search range are reported. For each
potential oscillation frequency found, an additional analysis for estimating
the probenode amplitude is also performed. All frequency and amplitude
values are reported. The frequency value that has the largest predicted
amplitude is used as the starting point for the two-tier Newton nonlinear
oscillator analysis.
–2: A multipoint frequency-search stability analysis is performed. The
FSPTS search is executed, and all successful linear oscillation frequency
values found over the entire FSPTS search range are reported. For each
potential oscillation frequency found, an additional analysis for estimating
the probenode amplitude is also performed. All frequency and amplitude
values are reported. The analysis aborts without attempting the two-tier
Newton nonlinear oscillator analysis. By using STABILITY=–2, a check
can be made if any linear oscillation conditions are found, before
attempting the nonlinear oscillator analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBOSC
Argument
Description
SWEEP
Type of sweep. You can sweep up to three variables. You can specify either
LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, OPTIMIZE, or MONTE.
Specify the nsteps, start, and stop frequencies using the following syntax for
each type of sweep:
■
■
■
■
■
■
■
■
SUBHARMS
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA=dataname
OPTIMIZE=OPTxxx
MONTE=val
Subharmonics in the analysis spectrum. The minimum non-DC frequency in
the analysis spectrum is f/subharms, where f is the frequency of oscillation.
Use this option if your oscillator circuit includes a divider or prescaler that
result in frequency terms that are subharmonics of the fundamental
oscillation frequency
Description
Use this command to invoke oscillator analysis on autonomous (oscillator)
circuits.
Examples
Example 1
Performs an oscillator analysis searching for frequencies in the vicinity of
900 MHz. This example uses nine harmonics with the probe inserted
between the gate and gnd nodes. The probe voltage estimate is 0.65 V.
.HBOSC tone=900MEG nharms=9 probenode=gate,gnd,0.65
Example 2
Performs an oscillator analysis searching for frequencies in the vicinity of
2.4 GHz. This example uses 11 harmonics with the probe inserted
between the drainP and drainN nodes. The probe voltage estimate is 1.0
V.
.HBOSC tone=2400MEG nharms=11
+ probenode=drainP,drainN,1.0 fspts=20,2100MEG,2700MEG
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
129
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBOSC
Another means to define the probenode information is through a zero-current
source. Examples 3 and 4 shows two methods define an equivalent .HBOSC
command.
Example 3
Method 1
.HBOSC tone = 2.4G nharms = 10
+ probenode = drainP, drainN, 1.0
+ fspts = 20, 2.1G, 2.7G
In Method 2, the PROBENODE information is defined by a current source in the
circuit. Only one such current source is needed, and its current must be 0.0
with the HBOSC PROBENODE voltage defined through its HBOSCVPROBE
property.
Example 4
Method 2
ISRC drainP drainN 0 HBOSCVPROBE = 1.0
.HBOSC tone = 2.4G nharms = 10
+ fspts = 20, 2.1G, 2.7G
See Also
.HB
.OPTION HBFREQABSTOL
.OPTION HBFREQRELTOL
.OPTION HBOSCMAXITER (or) HBOSC_MAXITER
.OPTION HBPROBETOL
.OPTION HBTRANFREQSEARCH
.OPTION HBTRANINIT
.OPTION HBTRANPTS
.OPTION HBTRANSTEP
.PRINT
.PROBE
130
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HBXF
.HBXF
Calculates transfer from the given source in the circuit to the designated output.
Syntax
.HBXF out_varfreq_sweep
Argument
Description
out_var
Specify i(2_port_elem) or V(n1<,n2>)
freq_sweep A sweep of type LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify
nsteps, start/stop times the syntax below for each type of sweep:
■
LIN nsteps start stop
DEC nsteps start stop
■
OCT nsteps start stop
■
POI nsteps freq_values
■
SWEEPBLOCK = BlockName
Specify the frequency sweep range for the output signal. HSPICE RF
determines the offset frequency in the input sidebands; for example,f1 =
abs(fout - k*f0) s.t. f1<=f0/2The f0 is the steady-state fundamental tone
and f1 is the input frequency.
■
Description
Calculates the transfer function from the given source in the circuit to the
designated output.
Examples
Here, trans-impedance from isrc to v(1)is calculated based on HB analysis.
.hb tones=1e9 nharms=4
.hbxf v(1) lin 10 1e8 1.2e8
.print hbxf tfv(isrc) tfi(n3)
See Also
.HB
.HBAC
.HBNOISE
.HBOSC
.SNXF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
131
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HDL
.HDL
Specifies the Verilog-A source name and path.
Syntax
.HDL "file_name" [module_name] [module_alias]
Argument
Description
file_name
Verilog-A or CML file.
module_name
Optional module name. If a module is specified, then only that
module is loaded from the specified Verilog-A or CML file. If the
module is not found or if the module specification is not uniquely
case-insensitive inside, then an error is generated. (HSPICE only).
module_alias
If specified (in addition to a module name), then that module is
loaded into the system using the alias in place of the module name
defined in the Verilog-A source file. Thereafter, any reference to the
module is made using its alias. The system behaves as if the
module had the alias as its module name. A module might be
loaded with any number of aliases in addition to being loaded
without an alias. This argument is useful when loading modules of
the same name from different files. See Example 4 below. (HSPICE
only)
Description
Use .HDL commands to specify the Verilog-A or compiled model library (CML)
source name and path within a netlist. The Verilog-A file is assumed to have
a *.va extension only when a prefix is provided. You can also use .HDL
commands in .ALTER blocks to vary simulation behavior. For example, to
compare multiple variations of Verilog-A modules.
In .MODEL commands you must add the Verilog-A type of model cards. Every
Verilog-A module can have one or more associated model cards. The type of
model cards should be the same as the Verilog-A module name. Verilog-A
module names cannot conflict with HSPICE built-in device keywords. If a
conflict occurs, HSPICE issues a warning message and the Verilog-A module
definition is ignored.
The module_name and module_alias arguments can be specified without
quotes or with single or double quotes. Any tokens after the module alias are
ignored.
132
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.HDL
The same Verilog-A case insensitivity rules used for module and parameter
names apply to both the module_name and module_alias arguments, and
the same module override logic applies.
Examples
Example 1 loads the res.va Verilog-A model file from the directory /myhome/
Verilog_A_lib.
Example 1
.HDL "/myhome/Verilog_A_lib/res.va"
Example 2 loads the va_models.va Verilog-A model file (not va_model file)
from the current working directory.
Example 2
.HDL "va_models"
Example 3 loads the module called va_amp from the amp_one.va file for the
first simulation run. For the second run, HSPICE loads the va_amp module
from the amp_two.va file.
Example 3
* simple .alter test
.hdl amp_one.va
v1 1 0 10
x1 1 0 va_amp
.tran 10n 100n
.alter alter1
.hdl amp_two.va
.end
See Also
.ALTER
.MODEL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
133
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IBIS
.IBIS
Provides IBIS functionality by specifying an IBIS file and component and
optional keywords.
Syntax
.IBIS 'ibis_name'
+ file='ibis_file_name'
+ component='component_name' [time_control=0|1]
+ [mod_sel='sel1=mod1,sel2=mod2,...']
+ [package=0|1|2|3] [pkgfile='pkg_file_name']
+ [typ={typ|min|max}]
+ [nowarn]
+ ...
Argument (Keyword) Description
ibis_name
Instance name of this ibis command.
file
Name of ibis (*ibs) file.
component or
cname
Component name.
time_control
Invokes an HSPICE time-control algorithm to achieve greater
accuracy for high speed digital signal buffers:
■
■
mod_sel
134
0 (default): Time step algorithm will not take effect.
1: Launches the time-step algorithm.
Assigns special model for model selector, here model selector
can be used for series model. If model selector is used for a pin
of a component, but mod_sel is not set in the .ibis command,
then the first model under the corresponding [Model Selector]
will be selected as default.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IBIS
Argument (Keyword) Description
package
When package equals:
0, then the package is not added into the component.
1, then RLC of [Package] (in the .ibs file) is added.
2, then RLC of [Pin] (in the .ibs file) is added.
3 (default), and if [Package Model] is defined, set package with
a package model.
If the [Package Model] is not defined, set the package with [Pin].
If the package information is not set in [Pin], set the package with
[Package] as a default.
You can define the [Package Model] in an IBIS file specified by
the file keyword or a PKG file specified by the pkgfile keyword.
The pkgfile keyword is useful only when package =3
typ
The value of the typ signifies a column in the IBIS file from which
the current simulation extracts data. The default is typ=typ. If min
or max data are not available, typ data are used instead.
nowarn
The nowarn keyword suppresses warning messages from the
IBIS parser.
Description
The general syntax above shows the .IBIS command when used with a
component. The optional keywords are in square brackets.
Examples
.ibis cmpnt
+ file = ’ebd.ibs’
+ component = ’SIMM’
+ hsp_ver=2002.4 nowarn package=2
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
135
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IBIS
This example corresponds to the following ebd.ibs file:
[Component]
SIMM
[Manufacturer]
TEST
[Package]
R_pkg
200m
NA
NA
L_pkg
7.0nH
NA
NA
C_pkg
1.5pF
NA
NA
|
[Pin]
signal_name
model_name
R_pin
|
1
ND1
ECL
40.0m
2n
0.4p
2
ND2
NMOS
50.0m
3n
0.5p
...................
L_pin
C_pin
Component cmpnt
buffer cmpnt_nd1
cmpnt_1
cmpnt_1_i
0.4p
40.0m
2n
gnd
buffer cmpnt_nd2
cmpnt_2
cmpnt_2_i
0.5p
50.0m
3n
gnd
Figure 8
Equivalent Circuit for IBIS Component Example
.IBIS cmpt1
+ file='example.ibs'
+ component='EXAMPLE'
+ mod_sel = 'DQ = DQ_FULL'
136
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IBIS
In the following example, the model DQ_FULL will be used for all pins that use
the model name DQ.The corresponding IBIS file, example.ibs, contains the
following [Model Selector] section:
|***********************MODEL SELECTOR***********************
|
Model Selector] DQ
|
DQ_FULL
Full-Strength IO Driver
DQ_HALF
54% Reduced Drive Strength IO Driver
*
See Also
.EBD
.PKG
IBIS Examples (/iob_ex1.sp) for demonstration files and see .IBIS
command use in ebd.sp and pinmap.sp
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
137
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IC
.IC
Sets transient initial conditions in HSPICE.
Syntax
.IC V(node1)=val1 V(node2)=val2 ... [subckt=sub_name]
Argument
Description
val1 ...
Specifies voltages. The significance of these voltages depends on
whether you specify the UIC parameter in the .TRAN command.
node1 ...
Node numbers or names can include full paths or circuit numbers.
subckt=sub_name
Initial condition is set to the specified node name(s) within all instances
of the specified subcircuit name. This subckt setting is equivalent to
placing the .IC statement within the subcircuit definition.
Description
Use the .IC command or the .DCVOLT command to set transient initial
conditions in HSPICE. How it initializes depends on whether the .TRAN
analysis command includes the UIC parameter. This command is less
preferred compared to using the.NODESET command in many cases.
When using the .IC command, forcing circuits are connected to the .IC nodes
for the duration of DC convergence. After DC convergence is obtained, the
forcing circuits are removed for all further analysis. The DC operating point for
each .IC'd node should be very close to the voltage specified in the .IC
command. If a node is not, then that node has a DC conductance to ground
comparable to GMAX. This is almost certainly an error condition. In the rare
case that it is not, GMAX can be increased to prevent appreciable current
division. Example: .OPTION GMAX=1000
Note:
In nearly all applications, .NODESET should be used to ensure a
true DC operating point is obtained. Intentionally floating (or very
high impedance) nodes should be set to a known good voltage
using .IC.
If you do not specify the UIC parameter in the .TRAN command, HSPICE
computes the DC operating point solution before the transient analysis. The
node voltages that you specify in the .IC command are fixed to determine the
DC operating point. They are used only in the first iteration to set an initial
guess for the DC operating point analysis. The .IC command is equivalent to
138
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IC
specifying the IC parameter on each element command, but is more
convenient.
If you specify the UIC parameter in the .TRAN command, HSPICE does not
calculate the initial DC operating point, but directly enters transient analysis.
When you use .TRAN UIC, the .TRAN node values (at time zero) are
determined by searching for the first value found in this order: from .IC value,
then IC parameter on an element command, then .NODESET value, otherwise
use a voltage of zero.
Note that forcing a node value of the dc operating point may not satisfy KVL
and KCL. In this event you may likely see activity during the initial part of the
simulation.This may happen if UIC is used and some node values left
unspecified, when too many (conflicting) .IC values are specified, or when
node values are forced and the topology changes. In this event you may likely
see activity during the initial part of the simulation. Forcing a node voltage
applies a fixed equivalent voltage source during DC analysis and transient
analysis removes the voltage sources to calculate the second and later time
points.
Therefore, to correct DC convergence problems use .NODESETs (without
.TRAN UIC) liberally (when a good guess can be provided) and use .ICs
sparingly (when the exact node voltage is known).
In addition, you can use wildcards in the .IC command. See Using Wildcards
on Node Names in the HSPICE User Guide: Simulation and Analysis.
Examples
Example 1
.IC V(11)=5 V(4)=-5 V(2)=2.2
Example 2
All settings in this statement are applied to subckt my_ff.
.IC V(in)=0.9 subckt=my_ff
See Also
.DCVOLT
.TRAN
.OPTION DCIC
.NODESET
.OPTION GMAX
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
139
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ICM
.ICM
Automatically creates port names that reference the pin name of an ICM model
and generate a series of element nodes on the pin.
Syntax
.ICM icmname
+ file='icmfilename'
+ model='icmmodelname'
Argument
Description
icmname
.ICM command card name.
icmfilename
Name of an *.icm file that contains an ICM model.
icmmodelname
Working model in an .icm file.
nodemapname
Name of the [ICM node map] keyword in an .icm file.
pinmapname
Name of the [ICM pin map] keyword in an .icm file.
pinname
Name of the first column of entries of the [ICM node map] or [ICM
pin map].
sidename
Name of the side subparameter
Description
Use this command to automatically create port names that reference the pin
name of an ICM model and generate a series of element (W/S/RLGCK) nodes
on the pin when one of the following conditions occur:
■
If the model is described using [Nodal Path Description]
'icmname'_'nodemapname'_'sidename'_'pinname'
■
If the model is described using [Tree Path Description]
'icmname'_'pinmapname'_'sidename'_'pinname'
Note:
140
If a side subparameter is not used in an ICM file, then
'sidename'_ (above) should be removed.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.ICM
Examples
.ICM icm1
+ file='test1.icm'
+ model='FourLineModel1'
The following example shows how to reference a pin of the ICM model in a
HSPICE netlist.
icm1_NodeMap1_SideName1_pin1, icm1_NodeMap2_SideName2_pin1,
icm1_NodeMap2_SideName2_pin2, ...
See Also
IBIS Examples for .ICM command usage (RLGC approach—/icm/
nodepath_rlgc/bga_1.sp), (S-element approach—/icm/nodepath_sele
test1.sp), (treepath—test1.sp), and treepath swath matrix expansion (/icm/
treepath_swath/complex.sp)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
141
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IF
.IF
Specifies conditions that determine whether HSPICE executes subsequent
commands in conditional block.
Syntax
.IF (condition1)...
+ [.ELSEIF (condition2)...]
+ [.ELSE ...]
.ENDIF
Argument
Description
condition1
Condition that must be true before HSPICE executes the commands
that follow the .IF command.
condition2
Condition that must be true before HSPICE executes the commands
that follow the .ELSEIF command. HSPICE executes the commands
that follow condition2 only if condition1 is false and condition2 is true.
Description
HSPICE executes the commands that follow the first.ELSEIF command only if
condition1 in the preceding .IF command is false and condition2 in the
first .ELSEIF command is true.
If condition1 in the .IF command and condition2 in the first .ELSEIF
command are both false, then HSPICE moves on to the next .ELSEIF
command if there is one. If this second .ELSEIF condition is true, HSPICE
executes the commands that follow the second .ELSEIF command, instead of
the commands after the first .ELSEIF command.
HSPICE ignores the commands in all false .IF and .ELSEIF commands, until
it reaches the first .ELSEIF condition that is true. If no .IF or .ELSEIF
condition is true, HSPICE continues to the .ELSE command.
.ELSE precedes one or more commands in a conditional block after the
last .ELSEIF command, but before the .ENDIF command. HSPICE executes
these commands by default if the conditions in the preceding .IF command
and in all of the preceding .ELSEIF commands in the same conditional block
all false.
The .ENDIF command ends a conditional block of commands that begins with
an .IF command.
142
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IF
For information on use of conditional blocks with the Exploration Block, see,
Specifying Constraints in the HSPICE User Guide: Simulation and Analysis.
Examples
.IF (a==b)
.INCLUDE /myhome/subcircuits/diode_circuit1
...
.ELSEIF (a==c)
.INCLUDE /myhome/subcircuits/diode_circuit2
...
.ELSE
.INCLUDE /myhome/subcircuits/diode_circuit3
...
.ENDIF
See Also
.ELSE
.ELSEIF
.ENDIF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
143
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.INCLUDE (or) .INC (or) .INCL
.INCLUDE (or) .INC (or) .INCL
Includes another netlist as a subcircuit of the current netlist.
Syntax
.INCLUDE ‘file_pathfile_name’
Argument
Description
file_path
Path name of a file for computer operating systems that support treestructured directories.
An include file can contain nested .INCLUDE calls to itself or to
another include file. If you use a relative path in a nested .INCLUDE
call, the path starts from the directory of the parent .INCLUDE file, not
from the current working directory. If the path starts from the current
working directory, HSPICE can also find the .INCLUDE file, but prints
a warning.
file_name
Name of a file to include in the data file. The file path, plus the file
name, can be up to 16 characters long. You can use any valid file name
for the computer’s operating system.
Description
Use this command to include another netlist in the current netlist. You can
include a netlist as a subcircuit in one or more other netlists. You must enclose
the file path and file name in single or double quotation marks. Otherwise, an
error message is generated. Any file name following an .INC command is case
sensitive beginning with the 2009.09 release. This command can be used as
part of a compressed (.gzip) netlist file.
Examples
.INCLUDE `/myhome/subcircuits/diode_circuit´
144
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IVTH
.IVTH
invokes the constant-current based threshold voltage characterization. The
threshold voltage reported by iVth characterization is defined as the MOSFET's
gate-to-source voltage at which the drain terminal current reaches the userdefined constant current value. The drain and body biases of the device are set
to their corresponding bias conditions in the circuit. For example, in DCOP, the
drain and body bias of the device is set to its operating point condition. in DC
Sweep or transient analysis, drain and body bias of the device is set to its
solution at each sweep or time point.
Syntax
.IVTH model_name Ivth0=val DW=val DL=val VDSMIN=val
[.OPTION SX_factor=x]
Argument
Description
model_name
Model name that iVth characterization applies to.
Ivth0=val
Constant drain terminal current density.
DW=val
Width offset for iVth current calculation.
DL=val
Length offset for iVth current calculation.
VDSMIN=val
User-defined minimum vds value.
.OPTION SX_factor A special option, .OPTION SX_factor, is provided to scale the
width and length specifically for iVth characterization.
Description
Use this command to enable constant current-based threshold voltage
characterization. The constant current for each MOSFET is given as follows:
Ivth=Ivth0 * (Wdrawn * SX_factor + DW)/(Ldrawn * SX_factor + DL)
VDSMIN provides a user-defined minimum Vds value and invokes a special
characterization method for small Vds bias to ensure continuation and
meaningful characterization result.
If VDSMIN is not given, the same iVth characterization methodology is applied
for all vds bias regions.If VDSMIN is given, and Vds is smaller than VDSMIN,
then:
1. Simulate Vth_op(Vdsmin) and Vth_ivth(Vdsmin)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
145
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.IVTH
where: Vth_op() is the threshold voltage acquired from model formulation, and
vth_ivth() is the threshold voltage acquired from iVth method.
2. Calculate DeltaVth = Vth_op(Vdsmin) - Vth_ivth(Vdsmin)
3. Simulate Vth_op(Vds)
4. Calculate Vth_ivth(Vds) = Vth_op(Vds) - DeltaVth
Multiple ivth commands can be added in a netlist to invoke characterization of
different models.
Examples
.ivth nch Ivth0=1.5e-7 DW=2e-8 DL=1e-8 VDSMIN=0.06
.ivth pch Ivth0=1e-7 DW=2e-8 DL=1e-8 VDSMIN=0.06
In OP analysis, a constant current based vth is reported in the OP output.
Inaddition, the element region operation check and Vod output are based on
the new vth.
During transient or DC analysis, template output of LX142(m*) or ivth(m*)
could be used for the new vth output.
146
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.JITTER
.JITTER
Computes jitter time interval error measurements from transient noise or nonrandom noise errors from transient analyses.
Syntax
Computation of TIE (time interval error)
.JITTER TRANNOISE TRIG OutputVar VAL=num|expression
+ TD=num|expression
Computation of deterministic jitter without random noise
.JITTER TRAN TRIG OutputVar VAL=num|expression
+ TD=num|expression
Argument
Description
TRIG
Repetitive trigger specification.
OutputVar
The output variable is expected to be an ideal clock reference.
VAL=num|expression The value can be a number or an expression.
TD
Amount of simulation time that must elapse before the
measurement is enabled. The time delay can be a number or an
expression.
Description
Use this command following a TRANNOISE analysis which used the
autocorrelation=1 keyword. The autocorrelation function is calculated at the
specified output. TIE measures the time-shift behavior relative to a reference
signal. The autocorrelation function is used for tracking the relative time-shift
behavior of the signal.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
147
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LAYERSTACK
.LAYERSTACK
Defines a stack of dielectric or metal layers.
Syntax
.LAYERSTACK sname [BACKGROUND=mname]
+ [LAYER=(mname,thickness) ...]
Argument
Description
sname
Layer stack name.
mname
Material name.
BACKGROUND Background dielectric material name. By default, the field solver
assumes AIR for the background.
thickness
Layer thickness.
Description
Use this command to define a stack of dielectric or metal layers. You must
associate each transmission line system with only one layer stack. However,
you can associate a single-layer stack with many transmission line systems.
In the layer stack:
■
Layers are listed from bottom to top.
■
Metal layers (ground planes) can be located only at the bottom, only at the
top, or both at the top and bottom.
■
Layers are stacked in the y-direction; the bottom of a layer stack is at y=0.
■
All conductors must be located above y=0.
■
Background material must be dielectric.
The following limiting cases apply to the .LAYERSTACK command:
■
Free space without ground:
.LAYERSTACK mystack
■
Free space with a (bottom) ground plane where a predefined metal name =
perfect electrical conductor (PEC):
.LAYERSTACK halfSpace PEC 0.1mm
148
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LAYERSTACK
See Also
.FSOPTIONS
.MATERIAL
.SHAPE
Transmission (W-element) Line Examples
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
149
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIB
.LIB
Creates and reads from libraries of commonly used commands, device models,
subcircuit analyses, and commands.
Syntax
Use the following syntax for library calls:
.LIB ‘[file_path] file_name’ entry_name
Use the following syntax to define library files:
.LIB entry_name1
. $ ANY VALID SET OF HSPICE STATEMENTS
.ENDL entry_name1
.LIB entry_name2
.
. $ ANY VALID SET OF HSPICE STATEMENTS
.ENDL entry_name2
.LIB entry_name3
.
. $ ANY VALID SET OF HSPICE STATEMENTS
.ENDL entry_name3
Argument
Description
file_path
Path to a file. Used where a computer supports tree-structured directories. When
the LIB file (or alias) is in the same directory where you run HSPICE RF you do not
need to specify a directory path; the netlist runs on any machine. Use “../” syntax
in the file_path to designate the parent directory of the current directory.
entry_name Entry name for the section of the library file to include. The first character of an
entry_name cannot be an integer. If more than one entry with the same name is
encountered in a file, only the first one is loaded.
file_name
Name of a file to include in the data file. The combination of filepath plus
file_name can be up to 256 characters long, structured as any filename that is
valid for the computer’s operating system. Enclose the file path and file name in
single or double quotation marks. Use “../” syntax in the filename to designate
the parent directory of the current directory.
Description
Use the .LIB call command to read from libraries of commonly used
commands, device models, subcircuit analyses, and commands (library calls)
in library files. Note that as HSPICE RF encounters each .LIB call name in the
150
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIB
main data file, it reads the corresponding entry from the designated library file,
until it finds an .ENDL command.
You can also place a .LIB call command in an .ALTER block.
To build libraries (library file definition), use the .LIB command in a library file.
For each macro in a library, use a library definition command (.LIB
entry_name) and an .ENDL command. The .LIB command begins the
library macro and the .ENDL command ends the library macro. The text after a
library file entry name must consist of HSPICE RF commands. Library calls can
call other libraries (nested library calls) if they are different files. You can nest
library calls to any depth. Use nesting with the .ALTER command to create a
sequence of model runs. Each run can consist of similar components by using
different model parameters without duplicating the entire input file.
The simulator uses the .LIB command and the .INCLUDE command to
access the models and skew parameters. The library contains parameters that
modify .MODEL commands.
You must enclose the file path and file name in single or double quotation
marks. Otherwise, an error message is generated. Any file name following
a .LIB command is case sensitive beginning with the 2009.09 release. To
terminate the .LIB command use .ENDL or .ENDL TT.
This command can be used as part of a compressed (.gzip) netlist file.
Examples
Example 1 is a simple library call.
Example 1
* Library call
.LIB 'MODELS' cmos1
Example 2 shows the syntax of using any valid set of RF commands.
Example 2
.LIB MOS7
$ Any valid set of HSPICE RF commands
.
.
.
.ENDL MOS7
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
151
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIB
Example 3 is an example of illegal nested .LIB commands for the file3
library.
Example 3
.LIB MOS7
...
.LIB 'file3' MOS7 $ This call is illegal in MOS7 library
...
.ENDL
Example 4 is a .LIB call command of model skew parameters and features
both worst-case and statistical distribution data. The statistical distribution
median value is the default for all non-Monte Carlo analyses. The model is in
the /usr/meta/lib/cmos1_mod.dat include file.
Example 4
.LIB TT
$TYPICAL P-CHANNEL AND N-CHANNEL CMOS LIBRARY
$ PROCESS: 1.0U CMOS, FAB7
$ following distributions are 3 sigma ABSOLUTE GAUSSIAN
.PARAM TOX=AGAUSS(200,20,3)
$ 200 angstrom +/- 20a
+ XL=AGAUSS(0.1u,0.13u,3)
$ polysilicon CD
+ DELVTON=AGAUSS(0.0,.2V,3)
$ n-ch threshold change
+ DELVTOP=AGAUSS(0.0,.15V,3)
$ p-ch threshold change
.INC ‘/usr/meta/lib/cmos1_mod.dat’
$ model include file
.ENDL TT
.LIB FF
$HIGH GAIN P-CH AND N-CH CMOS LIBRARY 3SIGMA VALUES
.PARAM TOX=220 XL=-0.03 DELVTON=-.2V
+ DELVTOP=-0.15V
.INC ‘/usr/meta/lib/cmos1_mod.dat’
$ model include file
.ENDL FF
In example 5, the .MODEL keyword (left side) equates to the skew parameter
(right side). A .MODEL keyword can be the same as a skew parameter.
Example 5
.MODEL NCH NMOS LEVEL=2 XL=XL TOX=TOX
+ DELVTO=DELVTON .....
.MODEL PCH PMOS LEVEL=2 XL=XL TOX=TOX
+ DELVTO=DELVTOP .....
152
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIB
See Also
.ALTER
.ENDL (or) .ENDL TT
.INCLUDE (or) .INC (or) .INCL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
153
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIN
.LIN
Extracts noise and linear transfer parameters for a general multiport network.
Syntax
Multiport Syntax
.LIN [sparcalc=[1|0] [modelname = modelname]]
+ [filename = filename]
+ [format=selem|citi|touchstone|touchstone2]
+ [noisecalc=[2|1|0] [gdcalc=[1|0]]
+ [mixedmode2port=dd|dc|ds|cd|cc|cs|sd|sc|ss]>
+ [dataformat=ri|ma|db]
Two-Port Syntax
.LIN [sparcalc=1|0 [modelname = modelname]]
+ [filename = filename]
+ [format=selem|citi|touchstone|touchstone2]
+ [noisecalc=1|0] [gdcalc=1|0]
+ [mixedmode2port=dd|dc|ds|cd|cc|cs|sd|sc|ss]
+ [dataformat=ri|ma|db] [FREQDIGIT=x] [SPARDIGIT=x]
+ [listfreq=(frequencies|none|all|freq1 freq2...)]
+ [listcount=num] [listfloor=val] [listsources=1|0|yes|no]
Argument
Description
sparcalc
If 1, extract S parameters (default).
modelname
Model name to be listed in the .MODEL command in the .sc# model
output file.
filename
Output file name (The default is netlist name).
format
Output file format:
■
■
■
noisecalc
154
selem is for S-element .sc# format, which you can include in the
netlist.
citi is CITIfile format.
touchstone and touchstone2: TOUCHSTONE v1.0 and v2.0 format,
respectively.
Specifies level of N-port noise wave correlation matrix extraction.
If 2, extract N noise parameters (perform multiport noise analysis). If 1,
extract noise parameters (perform 2-port noise analysis). Default is 0.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIN
Argument
Description
gdcalc
If 1, extract group delay (perform group delay analysis). Default is 0.
mixedmode2port
The mixedmode2port keyword describes the mixed-mode data map of
output mixed mode S-parameter matrix. The availability and default
value for this keyword depends on the first two port (P-element)
configuration as follows:
■
■
■
■
dataformat
case 1: p1=p2=single (standard mode P element)
available: ss
default: ss
case 2: p1=p2=balanced (mixed mode P element)
available: dd, cd, dc, cc
default: dd
case 3: p1=balanced p2=single
available: ds, cs
default: ds
case 4: p1=single p2=balanced
available: sd, sc
default: sd
The dataformat keyword describes the data format output to the .sc#/
touchstone/citi file.
■
dataformat=RI, real-imaginary. This is the default for the .sc#/citi file.
dataformat=MA, magnitude-phase. This is the default format for
touchstone file.
■
dataformat=DB, DB(magnitude)-phase.
HSPICE uses six digits for both frequency and S-parameters in
HSPICE generated data files (.sc#/touchstone/citifile). The number of
digits for noise parameters are five in .sc# and Touchstone files and six
in CITIfiles.
Note: The lower limit of DB output is -300.
■
FREQDIGIT
Sets the numerical precision (number of digits) for frequency output in
Touchstone, Citi, or sc# files. The default is 6.
SPARDIGIT
Sets the numerical precision (number of digits) for S parameter output
in Touchstone, Citi, or sc# files. The default is 6.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
155
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIN
Argument
Description
listfreq=
(none|all|freq1req2....)
Dumps the element noise figure contribution to the total NF in the *.lis
file. You can specify at which frequencies HSPICE dumps the element
noise figure contribution. The elements that contribute the largest noise
figure are dumped first. The frequency values can be specified by the
NONE or ALL keyword, which either dumps no frequencies or every
frequency defined in the AC sweep.
■
ALL: Output all of the frequency points (default, if LIST* is required).
NONE - Do not output any of the frequency points.
■
freq1 freq2...: Output the information on the specified frequency
points.
For example:
listfreq=none
■
listfreq=all
listfreq=1.0G
listfreq=1.0G 2.0G
listcount=num
Outputs the first few noise elements that make the biggest contribution
to NF. The number is specified by num. The default is to output all of the
noise element contribution to NF. The NF contribution is calculated with
the source impedance equal to the Zo of the first port.
listfloor=val
Lists elements whose noise contribution to NF (in dB) are higher than
value specified in dB to .lis file. Default is 0.
listsources=[1|0|yes|no] Defines whether or not to output the contribution of each noise source
of each noise element. Default is no/0.
Description
Use this command to extract noise and linear transfer parameters for a general
multiport network.
When used with P- (port) element(s) and .AC commands, .LIN makes
available a broad set of linear port-wise measurements:
156
■
standard and mixed-mode multiport S- (scattering) parameters
■
standard and mixed-mode multiport Y/Z parameters
■
standard mode multiport H-parameter
■
standard mode two-port noise parameters
■
standard and mixed-mode group delays
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LIN
■
standard mode stability factors
■
standard mode gain factors
■
standard mode matching coefficients
The .LIN command computes the S-(scattering), Y-(admittance), Z(impedance) parameters directly, and H-(hybrid) parameters directly based on
the location of the port (P) elements in your circuit, and the specified values for
their reference impedances. The .LIN command also supports mixed-mode
transfer parameters calculation and group delay analysis when used together
with mixed-mode P elements.
To calculate the insertion and return loss for the high speed differential signal
on my PCB board you can use the .LIN command with a port (P) element at
input and output, where Port=1 defines the input and Port=2 defines the output.
The return loss in dB is |S111(DB)| and the insertion loss in dB is
|S21(DB)|.
By default, the .LIN command creates a .sc# file with the same base name as
your netlist. This file contains S-parameter, noise parameter, and group delay
data as a function of the frequency. You can use this file as model data for the
S-element. Noise contributor tables are generated for every frequency point
and every circuit device. The last four arguments allow users to better control
the output information. If the LIST* arguments are not set, .LIN 2port noise
analysis will output to .lis file with the older format. If any of the LIST*
arguments is set, the output information follows the syntax noted in the
arguments section.
Examples
This example extracts linear transfer parameters for a general multiport
network, performs a 2-port noise analysis and a group-delay analysis for a
model named my_custom_model. The output is in the mydesign Touchstone
format output file. The data format in the Touchstone file is real-imaginary.
.LIN sparcalc=1 modelname=my_custom_model
+ filename=mydesign format=touchstone noisecalc=1
+ gdcalc=1 dataformat=ri
See Also
Filters Examples, fbpnet.sp, for a bandpass LCR filter demo using the .LIN
command
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
157
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LOAD
.LOAD
Uses the operating point information of a file previously created with a .SAVE
command.
Syntax
.LOAD [FILE=load_file] [RUN=PREVIOUS|CURRENT]
Argument
Description
load_file
Name of the file in which .SAVE saved an operating point for the
circuit under simulation.The format of the file name is design.ic#.
Default is design.ic0, where design is the root name of the design.
RUN
The format of file name is design.ic#. Used only outside of .ALTER
commands in a netlist that contains .ALTER commands.
■
■
PREVIOUS: Each .ALTER uses the saved operating point from the
previous .ALTER run in the current simulation run.
CURRENT: Each .ALTER uses the saved operating point from the
corresponding .ALTER run in the previous simulation run.
Description
Use this command to input the contents of a file that you stored using
the .SAVE command. Files stored with the .SAVE command contain operating
point information for the point in the analysis at which you executed .SAVE.
Do not use the .LOAD command for concatenated netlist files.
This command can be used as part of a compressed (.gzip) netlist file.
Examples
Example 1 loads a file name design.ic0, which you previously saved using
a .SAVE command.
Example 1
.SAVE FILE=design.ic0
.LOAD FILE=design.ic0
$load--design.ic0 save--design.ic0
.alter
...
$load--none
save--design.ic1
.alter
...
$load--none
save--design.ic2
.end
158
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LOAD
Example 2 runs a previously saved and loaded design.
Example 2
.SAVE FILE=design.ic
.LOAD FILE=design.ic RUN=PREVIOUS
$load--none
save--design.ic0
.alter
...
$load--design.ic0 save--design.ic1
.alter
...
$load--design.ic1 save--design.ic2
.end
Example 3 runs the current design.
Example 3
.SAVE FILE=design.ic
.LOAD FILE=design.ic RUN=CURRENT
$load--design.ic0 save--design.ic0
.alter
...
$load--design.ic1 save--design.ic1
.alter
...
$load--design.ic2 save--design.ic2
.end
See Also
.ALTER
.SAVE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
159
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LPRINT
.LPRINT
Produces output in VCD file format from transient analysis in HSPICE RF.
(Valid only for HSPICE RF.)
Syntax
.LPRINT (v1,v2) output_varable_list
Argument
Description
v1, v2
Threshold values for digital output. Values less than v1 are output
as digital 0. Values greater than 1 are output as digital 1.
output_varable_list Output variables to .PRINT. These are variables from a DC, AC,
TRAN, or NOISE analysis).
Description
Use this command to produce output in VCD file format from transient analysis.
Examples
In this example, the .LPRINT command sets threshold values to 0.5 and 4.5,
and the voltage level at voltage source VIN.
.OPTION VCD
.LPRINT (0.5,4.5) v(VIN)
See Also
.PRINT
160
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LSTB
.LSTB
Invokes linear loop stability analysis.
Syntax
Vxxx drv fbk 0
.LSTB mode=[single|diff|comm]
+ vsource=[vlstb|vlstbp,vlstbn]
.PRINT|PROBE AC
+ LSTB|LSTB(DB)|LSTB(M)|LSTB(P)|LSTB(R)|LSTB(I)
Argument
Description
Vxxx
The 0V voltage source(s) indicating the insertion point of test circuit. Note that
the direction of Vxxx is of significance in diff/comm mode analysis.
■
■
mode
■
■
■
Vsource
■
■
■
drv: Driving node (i.e., input of amplifier)
fbk: Feedback node (i.e., output of amplifier)
Single: (default) single-ended test.
Diff: differential mode test.
Comm: common mode test.
Vlstb: The only one vsource for single-ended mode test.
Vlstbp: One of the two vsources for differential or common mode test.
Vlstpn: The other one of the two vsources for differential or common mode
test.
LSTB
Output all results: dB, magnitude, phase, real and imaginary part of loop gain.
LSTB(x)
■
■
■
■
■
x=DB: Output the dB values of loop gain.
X=M: Output magnitude of loop gain.
X=P: Output phase of loop gain.
X=R: Output real part of loop gain.
X=I: Output imaginary part of loop gain.
Description
The .LSTB command measures the loop gain by successive injection
(Middlebrook’s Technique). A 0V voltage source is placed in series in the loop:
one pin of the voltage loop must be connected to the loop input, the other pin to
the loop output. The orientation of inserted voltage sources in differential and
common-mode testing is significant. It is required that the positive terminal of
both voltage sources go to the input of amplifier or go to the output of amplifier.
The first 3 characters of the mode type are effective (sin, dif or com). For single-
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
161
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LSTB
ended (default mode) test: place one 0V DC voltage source in series and
specify its name in the loop of interest, then add the .LSTB statement and
specify single as mode. For differential and common-mode loop analysis, set
diff or comm as the mode and specify the names of two 0V DC voltage
sources.
.MEASURE statements are supported similar to any ac output variables. The
feature can be used with .ALTER to generate multiple loop analyses. (See
examples below.)
The outputs for loop stability analysis are as follows:
■
The gain margin (GM), phase margin (PM), unity gain frequency (FU) and
gain at minimum frequency (ADC) are reported in the *.lis file.
■
The Loop Gain is reported to the *.cx# file, which is always produced for
.LSTB analysis. The *.cx# file is a general file for all the complex number
outputs. It contains the data for waveforms as complex vectors.
■
If you specify.probe ac lstb(db) lstb(mag) lstb(real)
lstb(imag) lstb(phase), the specific format of loop gain goes to the
*.ac# file for viewing.
■
If an *.ac# file is produced with .probe ac lstb, then both *.ac# and *.cx#
file could be used to view magnitude, phase, real, and imaginary versus
frequency as complex vectors.
Considerations regarding loop stability analysis include the following:
162
■
.LSTB analysis is based on a linearized circuit at a given DC operating
point. It does not guarantee a stable condition for large signal condition. As
a final stability check, designers should perform transient analysis; i.e.,inject
a slow sinusoid superimposed with a series of fast pulses into the loop; the
amount of ringing indicates the degree of stability for the circuit.
■
All other independent AC voltage sources are disabled automatically
when.LSTB is enabled.
■
.OPTION UNWRAP is set to 1 and if phase wrapping is found, the phase is
corrected by 180 degrees.
■
If phase/gain margin is not found in the given ac analysis frequency range,
a warning message is issued.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.LSTB
Examples
Example 1
This example shows a sample portion of a netlist where the first two lines
are the 0 voltage sources indicating the insertion point of circuit under
test; line 3 sets the .LSTB analysis using the differential mode and
specifies the two vsources; line 4 sets the .AC analysis, and the last three
lines specify post-processing (printing, plotting, and measurements).
V1 n1 n2 0
V2 n3 n4 0
.LSTB mode=diff vsource=v1,v2
.AC DEC 10 1K 1MEG
.PRINT AC LSTB(DB) LSTB(M) LSTB(P) LSTB(R) LSTB(I)
.PROBE AC LSTB(DB) LSTB(M) LSTB(P) LSTB(R) LSTB(I)
.MEASURE AC phase_margin FIND LSTB(P) when LSTB(DB)=0
Example 2
The .MEASURE statement is supported such as any common ac output
variable.
.measure ac phase_margin FIND lstb(P) when lstb(db)=0
.measure ac integ1 INTEGRAL lstb(P) FROM=1k TO=100k
Example 3
.measure
.measure
.measure
.measure
In this example, the lstb scalars are measured in which lstb is the type
name, out1-out4 are names for output, followed by scalar variable
keywords:
lstb out1 gain_margin
lstb out2 phase_margin
lstb out3 unity_gain_freq
lstb out4 loop_gain_minifreq
Example 4
A series of loop stability analyses are supported by the .alter command.
V3 n3 n4 0
.lstb mode=single vsource=V3
.alter
V4 n5 n6 0
V5 n7 n8 0
.lstb mode=common vsource=v4, v5
See Also
.AC
.ALTER
.MEASURE LSTB
.PRINT
.PROBE
.OPTION UNWRAP
Using .LSTB for Loop Stability Analysis
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
163
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MACRO
.MACRO
Defines a subcircuit in your netlist.
Syntax
.MACRO subckt_namen1 [n2n3...] [parnam=val]
.EOM
Argument
Description
subckt_nam
reference name for the subcircuit model call.
n1 ...
Node numbers for external reference; cannot be the ground node
(zero). Any element nodes that are in the subcircuit, but are not in
this list strictly local with three exceptions:
■
■
■
Ground node (zero).
Nodes assigned using BULK=node in MOSFET or BJT models.
Nodes assigned using the .GLOBAL command.
parnam
Parameter name set to a value. Use only in the subcircuit. To
override this value, assign it in the subcircuit call or set a value in
a .PARAM command.
SubDefaultsList
SubParam1=Expression
[SubParam2=Expression...]
Description
Use this command to define a subcircuit in your netlist (effectively the same as
the .SUBCKT command). You can create a subcircuit description for a
commonly used circuit and include one or more references to the subcircuit in
your netlist. Use the .EOM command to terminate a .MACRO command.
Examples
Example 1 defines two subcircuits: SUB1 and SUB2. These are resistor divider
networks, whose resistance values are parameters (variables). The X1, X2,
164
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MACRO
and X3 commands call these subcircuits. Because the resistor values are
different in each call, these three calls produce different subcircuits.
Example 1
*FILE SUB2.SP TEST OF SUBCIRCUITS
.OPTION LIST ACCT
V1 1 0 1
.PARAM P5=5 P2=10
.SUBCKT SUB1 1 2 P4=4
R1 1 0 P4
R2 2 0 P5
X1 1 2 SUB2 P6=7
X2 1 2 SUB2
.ENDS
*
.MACRO SUB2 1 2 P6=11
R1 1 2 P6
R2 2 0 P2
.EOM
X1 1 2 SUB1 P4=6
X2 3 4 SUB1 P6=15
X3 3 4 SUB2
*
.MODEL DA D CJA=CAJA CJP=CAJP VRB=-20 IS=7.62E-18
+ PHI=.5 EXA=.5 EXP=.33
.PARAM CAJA=2.535E-16 CAJP=2.53E-16
.END
Example 2 implements an inverter that uses a Strength parameter. By default,
the inverter can drive three devices. Enter a new value for the Strength
parameter in the element line to select larger or smaller inverters for the
application.
Example 2
.SUBCKT Inv a y Strength=3
Mp1 <MosPinList> pMosMod L=1.2u W=’Strength * 2u’
Mn1 <MosPinList> nMosMod L=1.2u W=’Strength * 1u’
.ENDS
...
xInv0 a y0 Inv
$ Default devices: p device=6u,
$ n device=3u
xInv1 a y1 Inv Strength=5
$ p device=10u, n device=5u
xInv2 a y2 Inv Strength=1
$ p device= 2u, n device=1u
...
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
165
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MACRO
See Also
.ENDS
.EOM
.SUBCKT
166
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MALIAS
.MALIAS
Assigns an alias to a diode, BJT, JFET, or MOSFET model that you defined in
a .MODEL command.
Syntax
.MALIAS model_name=alias_name1 [alias_name2 ...]
Argument
Description
model_name
Model name defined in the .MODEL card
alias_name1...
Alias that an instance (element) of the model references
Description
Use this command to assign an alias (another name) to a diode, BJT, JFET, or
MOSFET model that you defined in a .MODEL command.
.MALIAS differs from .ALIAS in two ways:
■
A model can define the alias in an .ALIAS command, but not the alias in
a .MALIAS command. The .MALIAS command applies to an element (an
instance of the model), not to the model itself.
■
The .ALIAS command works only if you include .ALTER in the netlist. You
can use .MALIAS without .ALTER.
You can use .MALIAS to alias to a model name that you defined in a .MODEL
command or to alias to a subcircuit name that you defined in a .SUBCKT
command. The syntax for .MALIAS is the same in either usage.
Note:
The .MALIAS command is supported for diode, BJT, JFET, and
MOSFET models in .Global_Variation and
.Local_Variation blocks.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
167
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MALIAS
Examples
■
zendef is a diode model
■
zen and zend are its aliases.
■
The zendef model points to both the zen and zend aliases.
*file: test malias statement
.OPTION acct tnom=50 list gmin=1e-14 post
.temp 0.0 25
.tran .1 2
vdd 2 0 pwl 0 -1 1 1
d1 2 1 zend dtemp=25
d2 1 0 zen dtemp=25
* malias statements
.malias zendef=zen zend
* model definition
.model zendef d (vj=.8 is=1e-16 ibv=1e-9 bv=6.0 rs=10
+ tt=0.11n n=1.0 eg=1.11 m=.5 cjo=1pf tref=50)
.end
See Also
.ALIAS
.MODEL
168
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MATERIAL
.MATERIAL
Specifies material to be used with the HSPICE field solver.
Syntax
.MATERIAL mname METAL|DIELECTRIC [ER=val]
+ [UR=val] [CONDUCTIVITY=val] [LOSSTANGENT=val]
+ ROUGHNESS=val
Argument
Description
mname
Material name.
METAL|DIELECTRIC Material type: METAL or DIELECTRIC.
ER
Dielectric constant (relative permittivity).
UR
Relative permeability.
CONDUCTIVITY
Static field conductivity of conductor or lossy dielectric (S/m).
LOSSTANGENT
Alternating field loss tangent of dielectric (tan δ ).
ROUGHNESS
RMS surface roughness height, used when scaling the field
solver.
Description
The field solver assigns the following default values for metal:
CONDUCTIVITY=-1 (perfect conductor), ER=1, UR=1.
PEC (perfect electrical conductor) is a predefined metal name. You cannot
redefine its default values.The field solver assigns default values for dielectrics:
■
CONDUCTIVITY=0 (lossless dielectric)
■
LOSSTANGENT=0 (lossless dielectric)
■
ER=1
■
UR=1
AIR is a predefined dielectric name. You cannot redefine its default values.
Because the field solver does not currently support magnetic materials, it
ignores UR values.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
169
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MATERIAL
See Also
.LAYERSTACK
.FSOPTIONS
Transmission (W-element) Line Examples
170
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (or) .MEAS
.MEASURE (or) .MEAS
Modifies information to define the results of successive simulations.
Syntax
See the links below for the various syntaxes.
Description
Use this command to modify information and to define the results of successive
HSPICE simulations. The .MEASURE command prints user-defined electrical
specifications of a circuit. Optimization uses .MEASURE commands extensively.
You can shorten the command name to .MEAS. The specifications include:
■
Propagation
■
Delay
■
RIse time
■
Fall time
■
Peak-to-peak voltage
■
Minimum and maximum voltage over a specified period
■
Other user-defined variables
You can also use .MEASURE with either the error function (ERRfun) or GOAL
parameter to optimize circuit component values, and to curve-fit measured data
to model parameters.
The .MEASURE command can use several different formats, depending on the
application. You can use it for DC sweep, and AC or transient analyses.
Note:
If a .measure command uses the result of previous .meas
command, then the calculation starts when the previous result is
found. Until the previous result is found, it outputs zero.
Examples
To measure the difference between two different nodes in a dc analysis:
.MEAS dc V1 MAX V(1)
.MEAS dc V2 MAX V(2)
.MEAS VARG PARAM="(V2 - V1)"
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
171
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (or) .MEAS
See Also
.MEASURE (Rise, Fall, Delay, and Power Measurements)
.MEASURE (FIND and WHEN)
.MEASURE (Equation Evaluation/Arithmetic Expression)
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
.MEASURE (Integral Function)
.MEASURE (Derivative Function)
.MEASURE (Error Function)
.MEASURE (Pushout Bisection)
.MEASURE (ACMATCH)
.MEASURE (DCMATCH)
.MEASURE FFT
.MEASURE LSTB
.AC
.DC
.DCMATCH
.DOUT
.OPTION NCWARN
.OPTION MEASFAIL
.OPTION MEASFILE
.OPTION MEASOUT
.PRINT
.PROBE
.STIM
.TRAN
Measuring the Value of MOSFET Model Card Parameters
172
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Rise, Fall, Delay, and Power Measurements)
.MEASURE (Rise, Fall, Delay, and Power
Measurements)
Measures independent-variable differentials such as rise time, fall time, and
slew rate.
Syntax
Trigger and Target Subcommands
The following are parameters for the TRIG and TARG subcommands.
.MEASURE [DC|AC|TRAN] ResultName TRIG TrigSpec TARG TargSpec
+ [GOAL=val] [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
The input syntax for delay, rise time, and fall time in HSPICE RF is:
.MEASURE [TRAN] varnameTRIG_SPECTARG_SPEC
In this syntax, varname is the user-defined variable name for the measurement
(the time difference between TRIG and TARG events). The input syntax for
TRIG_SPEC and TARG_SPEC is:
TRIG var VAL=val [TD=time] [CROSS=c|LAST]
+ [RISE=r|LAST] [FALL=f|LAST][TRIG AT=time]
TARG var VAL=val [TD=time-delay] [CROSS=c|LAST]
+ [RISE=r|LAST] [FALL=f|LAST] [REVERSE][TARG AT=time]
Argument
Description
DC | AC | TRAN Analysis type of the measurement. If you omit this parameter,
HSPICE uses the last analysis mode that you requested.
result
Name associated with the measured value in the HSPICE output,
can be up to 16 characters long. This example measures the
independent variable, beginning at the trigger and ending at the
target:
■
Transient analysis measures time.
AC analysis measures frequency.
■
DC analysis measures the DC sweep variable.
If simulation reaches the target before the trigger activates, the
resulting value is negative.Do not use DC, TRAN, or AC as the result
name.
■
TRIG
Beginning of trigger specifications.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
173
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Rise, Fall, Delay, and Power Measurements)
Argument
Description
TARG
Beginning of the target specification.
TrigSpec
OutputVar VAL={Number|'Expression'} [TD={Numeric|'Expression'}]
where: NumericExpression=
{FloatingPointNumber|'AlgebraicExpression'} See Using Algebraic
Expressions for information on algebra in output statements.
TargSpec
OutputVar VAL={Numeric|'Expression'} [TD={Number|'Expression'}]
where: NumericExpression:=
{FloatingPointNumber|'AlgebraicExpression'} See Using Algebraic
Expressions for information on algebra in output statements. If a
time-delay is not specified for the Target, the TD is inherited from the
Trigger value.
GOAL
Desired measure value in ERR calculation for optimization. To
calculate the error, the simulation uses the equation:
ERRfun = ( GOAL – result ) ⁄ GOAL .
MINVAL
If the absolute value of GOAL is less than MINVAL, the MINVAL
replaces the GOAL value in the denominator of the ERRfun
expression. Used only in ERR calculation for optimization. The
default is 1.0e-12.
WEIGHT
Multiplies the calculated error by the weight value. Used only in ERR
calculation for optimization. The default is 1.0.
PRINT
■
■
174
print=0 prevents the printing a measure result into the measure
output file
print=1 (Default) prints the measure result into the output file
trig_var
Value of trig_var, which increments the counter by one for crossings,
rises, or falls. See Using Algebraic Expressions for information on
algebra in output statements.
trig_var
Specifies the name of the output variable that determines the logical
beginning of a measurement. If HSPICE reaches the target before
the trigger activates, .MEASURE reports a negative value. See
Using Algebraic Expressions for information on algebra in output
statements.
REVERSE
Allows trigger time to come before target time when added to the
command.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Rise, Fall, Delay, and Power Measurements)
Argument
Description
TD
Amount of simulation time that must elapse before HSPICE enables
the measurement. Simulation counts the number of crossings, rises,
or falls only after the time_delay value. Default trigger delay is zero.
If a time-delay is not specified for the Target, the TD is inherited from
the Trigger value.
AT=val
Special case for trigger specification. val is:
■
Time for TRAN analysis.
Frequency for AC analysis.
■
Parameter for DC analysis.
■
SweepValue from .DC mismatch analysis.
The trigger determines where measurement takes place.
■
Description
Use the Rise, Fall, and Delay form of the .MEASURE command to measure
independent-variable (time, frequency, or any parameter or temperature)
differentials such as rise time, fall time, slew rate, or any measurement that
requires determining independent variable values. This format specifies TRIG
and TARG subcommands. These two commands specify the beginning and end
of a voltage or current amplitude measurement.
Examples
Example 1
HSPICE automatically measures T_prop using the .MEASURE
command. This reference file contains .MEAS commands for rising edge
and falling edge measurements. The time delay is measured and saved
during simulation in an *.mt0 file. Note that if a falling edge simulation is
run, the rising edge measurements are invalid. Similarly, if a rising edge
simulation is run, the falling edge measurements are invalid. (Remember
this when referring to the *.mt0 file after a simulation.) In this sample
file, .MEASURE statements are provided to measure T_prop from the
ref_50pf waveform to each of ten loads. Since each load is measured, the
worst-case T_prop for a given configuration can be quickly determined by
finding the largest value. The .MEASURE commands work by “triggering”
on the ref_50pf signal as it crosses 1.5 volts, and ending the
measurement when the “target” waveform, crosses the specified voltage
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
175
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Rise, Fall, Delay, and Power Measurements)
for the last time. For rising edge measurements, this value is 2.0 Volts.
For falling edge measurements, the value is 0.8 Volt. Examples from a
sample file are listed here.
***************************************************************
*
Rising edge T_prop measurements
*
***************************************************************
.MEAS tran tr1_val TRIG V(ref_50pf) val=1.5v td=’per/2’ cross=1
+ TARG V(load1) val=2.0v rise=last
.MEAS tran tr2_val TRIG B(ref_50pf) val=1.5v td=’per/2’ cross=1
+TARG V(load2) val=2.0v rise=last
.
.
.
.MEAS tran tr10_val TRIG V(ref_50pf) val=1.5v td=’per/2 cross=1
+ TARG V(load10) val=2.0v rise=last
***************************************************************
*
Falling edge T_prop measurements
*
***************************************************************
.MEAS tran tf1_val TRIG V(ref_50pf val=1.5v td=’per/2’ cross=1
+TARG V(load1) val=0.8v fall=last
.
.
.
.MEAS tran tf10_vasl TRIG V(ref_50pf) vbal=1.5v td=’per/2’ cross=1
+ TARFG V(load10) val=0.8v fall=last
Example 2
Measures the propagation delay between nodes 1 and 2 for a
transient analysis. HSPICE measures the delay from the second
rising edge of the voltage at node 1 to the second falling edge of
node 2. Measurement begins when the second rising voltage at
node 1 is 2.5 V and ends when the second falling voltage at node
2 is 2.5 V. The TD=10n parameter counts the crossings after 10 ns
have elapsed. HSPICE prints results as tdlay=value.
* Example of rise/fall/delay measurement
.MEASURE TRAN tdlay TRIG V(1) VAL=2.5 TD=10n
+ RISE=2 TARG V(2) VAL=2.5 FALL=2
176
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Rise, Fall, Delay, and Power Measurements)
In Example 3, TRIG AT=10n starts measuring time at t=10 ns in the
transient analysis. The TARG parameters terminate time measurement when
V(IN) = 2.5 V on the third crossing. pwidth is the printed output variable.
If you use the .TRAN analysis command with a .MEAS command, do not use a
non-zero start time in the .TRAN command to avoid incorrect .MEAS results.
Example 3
.MEASURE TRAN riset TRIG I(Q1) VAL=0.5m RISE=3
+ TARG I(Q1) VAL=4.5m RISE=3
* Rise/fall/delay measure with TRIG and TARG specs
.MEASURE pwidth TRIG AT=10n TARG V(IN) VAL=2.5
+ CROSS=3
Example 4 shows a target delayed until the trigger time before the target counts
the edges.
Example 4
.MEAS TRAN TDEL12 TRIG V(signal1) VAL='VDD/2'
+ RISE=10 TARG V(signal2) VAL='VDD/2' RISE=1 TD=TRIG
By using the cross keyword, Example 4 calculates the final settled value when
you don't know how many times the signal crosses the final value.
Example 5
.meas tran tim2 when v(out)='final_value' cross=last
In Example 6, print=0 prevents the printing of Vmax to the *.mt0 and *.lis
files. Delay will be output into *.mt# file and *.lis file.
Example 6
.meas tran Vmax max v(out) print=0
.meas tran delay trig V(in) val=’vmax/2’ rise=1 targ v(out)
+ val=’vmax/2’ rise=1
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
Filters Examples, fbp_1.sp, for a bandpass LCR filter measurement demo
netlist
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
177
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (FIND and WHEN)
.MEASURE (FIND and WHEN)
Measures independent and dependent variables (as well as derivatives of
dependent variables if a specific event occurs).
Syntax
.MEASURE [DC|AC|TRAN] result WHEN out_var=val [TD=val]
+ [FROM=val] [TO=val]
+ [RISE=r|LAST][FALL=f|LAST][CROSS=c|LAST][REVERSE]
+ [GOAL=val] [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC|AC|TRAN] result
+ WHEN out_var1=out_var2 [TD=val] [RISE=r|LAST]
+ [FALL=f|LAST] [CROSS=c|LAST] [GOAL=val] [MINVAL=val]
+ [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC|AC|TRAN] result FIND out_var1
+ WHEN out_var2=val [TD=val] [FROM=val] [TO=val]
+ [RISE=r|LAST][FALL=f|LAST] [CROSS=c|LAST] [REVERSE]
+ [GOAL=val][MINVAL=val] [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC|AC|TRAN] result FIND out_var1
+ WHEN out_var2=out_var3 [TD=val]
+ [RISE=r|LAST] [FALL=f|LAST] [REVERSE] [CROSS=c|LAST]
+ [GOAL=val] [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC|AC|TRAN] result FIND out_var1
+ AT=val [FROM=val] [TO=val] [GOAL=val][MINVAL=val]
+ [WEIGHT=val] [PRINT 0|1]
Argument
Description
DC | AC | TRAN Analysis type of the measurement. If you omit this parameter,
HSPICE uses the last analysis mode that you requested.
178
result
Name of a measured value in the HSPICE output.
WHEN
WHEN function.
out_var(1,2,3)
Variables that establish conditions to start a measurement.
TD
Time at which measurement starts.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (FIND and WHEN)
Argument
Description
FROM... TO...
Allows adding multiple trigger conditions to some WHEN
measurements.
CROSS=c
RISE=r
FALL=f
Numbers indicate which CROSS, FALL, or RISE event to measure.
For example:
.meas tran tdlay trig v(1) val=1.5 td=10n
+ rise=2 targ v(2) val=1.5 fall=2
In this example, rise=2 specifies the measure of the v(1) voltage only
on the first two rising edges of the waveform. The value of these first
two rising edges is 1. However, trig v(1) val=1.5 indicates to trigger
when the voltage on the rising edge voltage is 1.5, which never
occurs on these first two rising edges. So the v(1) voltage
measurement never finds a trigger.
RISE=r, the WHEN condition is met and measurement occurs after
the designated signal has risen r rise times.
FALL =f, measurement occurs when the designated signal has fallen
f fall times.
A crossing is either a rise or a fall so for CROSS=c, measurement
occurs when the designated signal has achieved a total of c crossing
times as a result of either rising or falling.
For TARG, the LAST keyword specifies the last event.
LAST
HSPICE measures when the last CROSS, FALL, or RISE event
occurs.
■
CROSS=LAST, measurement occurs the last time the WHEN
condition is true for a rising or falling signal.
■
FALL=LAST, measurement occurs the last time the WHEN
condition is true for a falling signal.
■
RISE=LAST, measurement occurs the last time the WHEN
condition is true for a rising signal.
LAST is a reserved word; you cannot use it as a parameter name in
the above .MEASURE commands.
REVERSE
Allows FALL to precede RISE in specified .MEAS commands, when
declared.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
179
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (FIND and WHEN)
Argument
Description
GOAL
Desired .MEASURE value. Optimization uses this value in ERR
calculation. The following equation calculates the error:
ERRfun = ( GOAL – result ) ⁄ GOAL
In HSPICE RF output you cannot apply .MEASURE to waveforms
generated from another .MEASURE command in a parameter
sweep.
MINVAL
If the absolute value of GOAL is less than MINVAL, then MINVAL
replaces the GOAL value in the denominator of the ERRfun
expression. Used only in ERR calculation for optimization. The
default is 1.0e-12.
WEIGHT
Calculated error multiplied by the weight value. Used only in ERR
calculation for optimization. The default is 1.0.
PRINT
■
■
print=0 prevents the printing a measure result into the measure
output file
print=1 (Default) prints the measure result into the output file
FIND
FIND function.
AT=val
Special case for trigger specification. val is:
■
Time for TRAN analysis.
Frequency for AC analysis.
■
Parameter for DC analysis.
■
SweepValue from .DC mismatch analysis.
The trigger determines where measurement takes place.
■
Description
The FIND and WHEN functions of the .MEASURE command measure:
180
■
Any independent variables (time, frequency, parameter).
■
Any dependent variables (voltage or current for example).
■
A derivative of a dependent variable if a specific event occurs.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (FIND and WHEN)
Examples
Calculating Voltage
In Example 1, the first measurement, TRT, calculates the difference between
V(3) and V(4) when V(1) is half the voltage of V(2) at the last rise event.
The second measurement, STIME, finds the time when V(4) is 2.5V at the third
rise-fall event. A CROSS event is a rising or falling edge.
Example 1
* MEASURE statement using FIND/WHEN
.MEAS TRAN TRT FIND PAR(‘V(3)-V(4)’)
+ WHEN V(1)=PAR(‘V(2)/2’) RISE=LAST
.MEAS STIME WHEN V(4)=2.5 CROSS=3
Using a DC Sweep Variable: By adding par() to the sweep variable it can be
used in a .MEASURE command.
Example 2
* sweep measure
v0 1 0 3
r0 1 0 x
.dc x 1 5 1
.meas res find par(x) when i(r0)=2
.end
Example 3 calculates capacitance from node to node:
Example 3
.meas tran pct_5 when v(out)='vddr*0.05' rise=1
.meas tran pct_95 when v(out)='vddr*0.95' rise=1
.meas tran avg_rout_n avg par('v(out)/i(xinv.mn)')
+ from=pct_5 to=pct_95
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
181
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Continuous Results)
.MEASURE (Continuous Results)
Measures continuous results for TRIG-TARG and Find-When functions.
Syntax
.MEASURE [DC_CONT|AC_CONT|TRAN_CONT] result TRIG … TARG …
+ [GOAL=val] [MINVAL=val] [WEIGHT=val][PRINT 0|1]
.MEASURE [DC_CONT|AC_CONT|TRAN_CONT] result
+ WHEN out_var=val [TD=val]
+ [RISE=r | LAST] [FALL=f| LAST][CROSS=c | LAST]
+ [GOAL=val] [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC_CONT|AC_CONT|TRAN_CONT] result
+ WHEN out_var1=out_var2 [TD=val]
+ [RISE=r | LAST] [FALL=f | LAST] [CROSS=c | LAST]
+ [GOAL=val] [MINVAL=val] [WEIGHT=val]
.MEASURE [DC_CONT|AC_CONT|TRAN_CONT] result FIND out_var1
+ WHEN out_var2=val [TD=val] [RISE=r | LAST]
+ [FALL=f | LAST] [CROSS=c| LAST] [GOAL=val]
+ [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC_CONT|AC_CONT|TRAN_CONT] result FIND out_var1
+ WHEN out_var2=out_var3 [TD=val] [RISE=r | LAST]
+ [FALL=f | LAST] [CROSS=c | LAST] [GOAL=val]
+ [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
182
Argument
Description
DC_CONT
AC_CONT
TRAN_CONT
Analysis type of the continuous measurement.
result
Name of a measured value in the HSPICE output.
TRIG...
Beginning of trigger specifications.
TARG...
Beginning of the target specification.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Continuous Results)
Argument
Description
GOAL
Desired .MEASURE value. Optimization uses this value in ERR calculation.
The following equation calculates the error:
ERRfun = ( GOAL – result ) ⁄ GOAL
In HSPICE RF output you cannot apply .MEASURE to waveforms
generated from another .MEASURE command in a parameter sweep.
MINVAL
If the absolute value of GOAL is less than MINVAL, then MINVAL replaces
the GOAL value in the denominator of the ERRfun expression. Used only in
ERR calculation for optimization. The default is 1.0e-12.
WEIGHT
Calculated error multiplied by the weight value. Used only in ERR
calculation for optimization. The default is 1.0.
PRINT
■
■
print=0 prevents the printing a measure result into the measure output
file
print=1 (Default) prints the measure result into the output file
WHEN
WHEN function.
out_var(1,2,3)
Variables that establish conditions to start a measurement.
TD
Time at which measurement starts.
CROSS=c
RISE=r FALL=f
Numbers indicate which CROSS, FALL, or RISE event to measure. For
example:.meas tran tdlay trig v(1) val=1.5 td=10n + rise=2
targ v(2) val=1.5 fall=2 In this example, rise=2 specifies the
measure of the v(1) voltage only on the first two rising edges of the
waveform. The value of these first two rising edges is 1. However, trig v(1)
val=1.5 indicates to trigger when the voltage on the rising edge voltage is
1.5, which never occurs on these first two rising edges. So the v(1) voltage
measurement never finds a trigger.RISE=r, the WHEN condition is met and
measurement occurs after the designated signal has risen r rise times.FALL
=f, measurement occurs when the designated signal has fallen f fall times.A
crossing is either a rise or a fall so for CROSS=c, measurement occurs
when the designated signal has achieved a total of c crossing times as a
result of either rising or falling. For TARG, the LAST keyword specifies the
last event.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
183
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Continuous Results)
Argument
Description
LAST
HSPICE measures when the last CROSS, FALL, or RISE event occurs.
■
CROSS=LAST, measurement occurs the last time the WHEN condition
is true for a rising or falling signal.
■
FALL=LAST, measurement occurs the last time the WHEN condition is
true for a falling signal.
■
RISE=LAST, measurement occurs the last time the WHEN condition is
true for a rising signal.
LAST is a reserved word; you cannot use it as a parameter name in the
above .MEASURE commands.
FIND
FIND function.
Description
Enables HSPICE to give multiple results during the measurement of DC, AC,
and transient analysis data. For example, it gives all the time points at which
two signals cross each other. Similar to HSIM, this command uses the same
syntax. The standalone measure utility also supports this feature. The
continuous measurement feature only applies to TRIG-TARG and Find-When
functions.
Examples
In Example 1, the .measure statement will continuously find the voltage out1
when the voltage value of node a1 reaches 2.5 starting from the first falling
edge.
Example 1
.measure tran_cont vout1 find v(out1) when v(a1)=2.5 fall=1
In Example 2, the .measure statement will continuously report the time when
the voltage value of node a1 reaches 2.5V, starting from the second falling
edge.
Example 2
.measure tran_cont cont_vout1 when v(a1)=2.5 fall=2
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
184
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Equation Evaluation/Arithmetic Expression)
.MEASURE (Equation Evaluation/Arithmetic
Expression)
Evaluates an equation that is a function of the results of previous .MEASURE
commands.
Syntax
.MEASURE [DC|TRAN|AC] result PARAM=’equation’
+ [GOAL=val] [MINVAL=val] [PRINT 0|1]
.MEASURE TRAN varname PARAM="expression"
Argument
Description
DC | AC | TRAN
Analysis type of the measurement. If you omit this parameter,
HSPICE uses the last analysis mode that you requested.
result
Name of a measured value in the HSPICE output.
PARAM=’equation’
Equation wrapped in single quotes, a function of the results of
previous .MEASURE commands.
GOAL
Desired .MEASURE value. In HSPICE RF output you cannot
apply .MEASURE to waveforms generated from
another .MEASURE command in a parameter sweep.
MINVAL
If the absolute value of GOAL is less than MINVAL, then
MINVAL replaces the GOAL value in the denominator of the
ERRfun expression. Used only in ERR calculation for
optimization. The default is 1.0e-12.
TRAN
Transient analysis results.
varname
Name of variable to be used in evaluation.
PARAM="expression" Arithmetic expression that uses results from other
prior .MEASURE commands.
Description
Use the Equation Evaluation form of the .MEASURE command to evaluate an
equation that is a function of the results of previous .MEASURE commands. The
equation must not be a function of node voltages or branch currents.
The expression option is an arithmetic expression that uses results from other
prior .MEASURE commands.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
185
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Equation Evaluation/Arithmetic Expression)
Expressions used in arithmetic expression must not be a function of node
voltages or branch currents. Expressions used in all other .MEASURE
commands can contain either node voltages or branch currents, but must not
use results from other .MEASURE commands.
When using formulas in a .MEAS command, use the PAR( ) keyword to
designate the formula.
Examples
In Example 1, he first two measurements, V3MAX and V2MIN, set up the
variables for the third .MEASURE command.
■
V3MAX is the maximum voltage of V(3) between 0ns and 100ns of the
simulation.
■
V2MIN is the minimum voltage of V(2) during that same interval.
■
VARG is the mathematical average of the V3MAX and V2MIN measurements.
Example 1
.MEAS TRAN V3MAX MAX V(3) FROM 0NS TO 100NS
.MEAS TRAN V2MIN MIN V(2) FROM 0NS TO 100NS
.MEAS VARG PARAM=‘(V2MIN + V3MAX)/2’
Example 2 illustrates use of the par() keyword to measure the integral of a
formula.
Example 2
.meas i1 integ par('v(a)+v(b)')
186
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and
RMS)
Reports statistical functions of the output variable (voltage, current, or power).
Syntax
.MEASURE [DC|AC|TRAN] result func out_var
+ [FROM=val] [TO=val] [GOAL=val] MINVAL=val]
+ [WEIGHT=val] [PRINT 0|1]
Argument
Description
DC|AC|TRAN Analysis type for the measurement. If you omit this parameter, HSPICE
defaults to the last analysis mode that you requested.
result
Name of the measured value in the output, can be up to 16 characters
long. The value is a function of the variable (out_var) and func.
func
Indicates one of the following measure function types:
■
■
■
■
■
■
■
AVG (average): Calculates the area under the out_var, divided by
the periods of interest.
INTEG (Integral function): Reports the integral of an output variable
over a specified period.
MIN (minimum): Reports the minimum value of the out_var over the
specified interval.
MAX (maximum): Reports the maximum value of the out_var over
the specified interval.
PP (peak-to-peak): Reports the maximum value, minus the
minimum value of the out_var over the specified interval.
RMS (root mean squared): Calculates the square root of the area
under the out_var2 curve, divided by the period of interest.
EM_AVG: Calculates the average electromigration current. For a
symmetric bipolar waveform, the current is: I_avg (0, T/2) - R*Iavg
(T/2, T), where R is the recovery factor specified using .option
em_recovery. Wildcards are also supported during this
measurement.
out_var
Name of any output variable whose function (func) the simulation
measures (voltage, current, or power). An output variable can be any
dependent variable (voltage, current, or power).
FROM
Initial value for the INTEG calculation.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
187
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
Argument
Description
TO
End of the INTEG calculation.
GOAL
.MEASURE value. Optimization uses this value for ERR calculation.
This equation calculates the error:
ERRfun = ( GOAL – result ) ⁄ GOAL
In HSPICE RF simulation output you cannot apply .MEASURE to
waveforms generated from another .MEASURE command in a
parameter sweep.
WEIGHT
Calculated error multiplied by the weight value. Used only in ERR
calculation for optimization. The default is 1.0.
PRINT
■
■
print=0 prevents the printing a measure result into the measure
output file
print=1 (Default) prints the measure result into the output file
Description
Average (AVG), EM_AVG,RMS, MIN, MAX, and peak-to-peak (PP) measurement
modes report statistical functions of the output variable, rather than analysis
values. Output variables are voltage, current, or power. Wildcards are
supported for the From-To functions for AVG, EM_AVG, RMS, MIN, MAX and PP
measurement (unlike other measurement functions).
AVG, RMS, and INTEG have no meaning in a DC data sweep so if you use them,
HSPICE issues a warning message.
Examples
Example 1
Calculates the average nodal voltage value for node 10 during the
transient sweep from the time 10ns to 55ns. It prints out the result as
avgval
.MEAS TRAN avgval AVG V(10) FROM=10ns TO=55ns
Example 2
Finds the maximum voltage difference between nodes 1 and 2 for the
time period from 15 ns to 100 ns.
.MEAS TRAN MAXVAL MAX V(1,2) FROM=15ns TO=100ns
188
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
Example 3
The first command finds the minimum voltage difference between nodes
1 and 2 over the time period 15 ns to 100 ns. The second command
measures the peak to peak current through transistor M1 from 10ns to
100ns.
.MEAS TRAN MINVAL MIN V(1,2) FROM=15ns TO=100ns
.MEAS TRAN P2PVAL PP I(M1) FROM=10ns TO=100ns
Example 4
The coefficient value is set by .option em_recovery=val. The
electromagnetic migration average is measured from 5 ns to 10.2 ns.
.option em_recovery=0.2
.measure tran vout_1 EM_AVG v(5) from=5ns to=10.2ns
Example 5
These commands measure result parameter currents over specified
ranges.
.measure tran em1 em_avg i(rload) from=1n to=3.5n
.measure tran em2 em_avg i(rload) from=4n to=9n
Example 6
Finds the average of all the positive currents (Ipos_avg) from 5ns to 50ns.
.MEASURE TRAN EM_AVG I(OUT) FROM=5N TO=50N
Example 7
The .MEASURE command calculates the RMS voltage of the OUT
node from 0ns to 10ns. It then labels the result RMSVAL.
.MEAS TRAN RMSVAL RMS V(OUT) FROM=0NS TO=10NS
Example 8
The .MEASURE command finds the maximum current of the VDD voltage
supply between 10ns and 200ns. The result is called MAXCUR.
.MEAS MAXCUR MAX I(VDD) FROM=10NS TO=200NS
Example 9
The .MEASURE command uses the ratio of V(OUT) and V(IN) to find the
peak-to-peak value in the interval of 0ns to 200ns.
.MEAS P2P PP PAR(‘V(OUT)/V(IN)’) FROM=0NS TO=200NS
Example 10 Power measurement supplied by source vdd
.MEAS P(VDD)
Example 11 Three commands measuring power
.MEAS TRAN avg_cur avg par('-I(vh)')
.MEAS TRAN total_cur integ par('-I(vh)') from=0n to=3n
.MEAS TRAN total_pwr PARAM='total_cur*V(vdda)'
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
189
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
.OPTION EM_RECOVERY
190
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Integral Function)
.MEASURE (Integral Function)
Reports the real time integration (instantaneous time integral) of an output
variable over a specified period.
Syntax
.MEASURE [DC|AC|TRAN] result INTEG[RAL] out_var
+ [FROM=val] [TO=val] [GOAL=val]
+ [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
Argument
Description
DC | AC | TRAN
Analysis type of the measurement. If you omit this parameter,
HSPICE uses the last analysis mode that you requested.
result
Name of a measured value in the HSPICE output.
INTEG
Integral function to find an output variable over a specified period.
outvar
Name of any output variable whose function the simulation
measures.
FROM
Initial value for the func calculation. For transient analysis, this
value is in units of time.
TO
End of the func calculation.
GOAL
Desired .MEASURE value.
In HSPICE RF output you cannot apply .MEASURE to waveforms
generated from another .MEASURE command in a parameter
sweep.
MINVAL
If the absolute value of GOAL is less than MINVAL, then MINVAL
replaces the GOAL value in the denominator of the ERRfun
expression. Used only in ERR calculation for optimization. The
default is 1.0e-12.
Description
The INTEGRAL function reports the integral of an output variable over a
specified period. The INTEGRAL function uses the same syntax as the AVG
(average), RMS, MIN, MAX and peak-to-peak (PP) measurement modes.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
191
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Integral Function)
Examples
This example calculates the integral of I(cload) from 10ns to 100ns.
.MEAS TRAN charge INTEG I(cload) FROM=10ns TO=100ns
The following .MEASURE command calculates the integral of I(R1) from 50ns
to 200ns.
.MEASURE TRAN integ_i INTEGRAL I(r1) FROM=50ns TO=200ns
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
192
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Derivative Function)
.MEASURE (Derivative Function)
Provides the derivative of an output or sweep variable.
Syntax
.MEASURE [DC|AC|TRAN result DERIV[ATIVE] out_var
+ [FROM=val] [TO=val] AT=val [GOAL=val] [MINVAL=val]
+ [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC|AC|TRAN] result DERIV[ATIVE] out_var
+ [FROM=val TO=val] WHEN var2=val [RISE=r|LAST]
+ [FALL=f|LAST] [CROSS=c|LAST] [TD=tdval] [GOAL=goalval]
+ [MINVAL=minval] [WEIGHT=val] [PRINT 0|1]
.MEASURE [DC|AC|TRAN] result DERIV[ATIVE] out_var
+ [FROM=val] [TO=val] WHEN var2=var3 [RISE=r|LAST]
+ [FALL=f|LAST] [CROSS=c|LAST] [TD=tdval]
+ [GOAL=val] [MINVAL=val] [WEIGHT=val] [PRINT 0|1]
Argument
Description
DC | AC | TRAN Analysis type of the measurement. If you omit this parameter, HSPICE uses
the last analysis mode that you requested.
result
Name of the measured value in the output.
DERIVATIVE
Derivative function.
out_var
Variable for which HSPICE finds the derivative.
FROM=val
TO=val
Specifies a range to measure, such as time window.
var(2,3)
Variables establish that conditions to start a measurement.
AT=val
Value of out_var at which the derivative is found.
GOAL
Specifies the desired .MEASURE value. Optimization uses this value for ERR
calculation. This equation calculates the error:
ERRfun = ( GOAL – result ) ⁄ GOAL
In HSPICE RF output you cannot apply .MEASURE to waveforms generated
from another .MEASURE command in a parameter sweep.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
193
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Derivative Function)
Argument
Description
MINVAL
If the absolute value of GOAL is less than MINVAL, MINVAL replaces the
GOAL value in the denominator of the ERRfun expression. Used only in ERR
calculation for optimization. The default is 1.0e-12.
WEIGHT
Calculates the error between result and GOAL by multiplied by the weight
value. Used only in ERR calculation for optimization. The default is 1.0.
WHEN
WHEN function.
RISE=r FALL=f
CROSS=c
Numbers indicate which occurrence of a CROSS, FALL, or RISE event starts
a measurement.
■
■
■
LAST
For RISE=r when the designated signal has risen r rise times, the WHEN
condition is met and measurement starts.
For FALL=f, measurement starts when the designated signal has fallen f fall
times.
A crossing is either a rise or a fall so for CROSS=c, measurement starts
when the designated signal has achieved a total of c crossing times as a
result of either rising or falling.
Last CROSS, FALL, or RISE event.
■
CROSS=LAST, measures the last time the WHEN condition is true for a
rising or falling signal.
■
FALL=LAST, measures the last time WHEN is true for a falling signal.
■
RISE=LAST, measures the last time WHEN is true for a rising signal.
LAST is a reserved word; do not use it as a parameter name in the
above .MEASURE commands.
TD
Time when measurement starts.
Description
The DERIV function provides the derivative of:
■
An output variable at a specified time or frequency.
■
Any sweep variable, depending on the type of analysis.
■
A specified output variable when some specific event occurs.
Examples
Example 1
Calculates the derivative of V(out) at 25 ns.
.MEAS TRAN slew rate DERIV V(out) AT=25ns
194
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Derivative Function)
Example 2
Calculates the derivative of VP(output)/360.0 when the frequency is 10
kHz.
.MEAS AC delay DERIV ’VP(output)/360.0’ AT=10khz
Example 3
Measures the derivative of a nodal waveform.
.MEAS DC result find v(in) when deriv v(out)= …
Example 4
If you plot result from the command you will get the dV(out)/dTemperature
vs Temperature plot.
.MEAS DC result deriv v(out) …
Example 5
Measures and finds when the maximum derivative of a signal occurs. The
example shows (1) a probe of the derivative of the signal, (2) the
maximum value of the derivative, and (3) when the maximum value of the
derivative occurred.
.probe dt=deriv("v(out)")
.meas m0 max par(dt)
.meas m1 when par(dt)=m0
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
195
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Error Function)
.MEASURE (Error Function)
Reports the relative difference between two output variables.
Syntax
.MEASURE [DC|AC|TRAN] result
+ ERRfun meas_varcalc_var
+ [MINVAL=val] [IGNOR|YMIN=val]
+ [YMAX=val] [WEIGHT=val] [FROM=val] [TO=val] [PRINT 0|1]
Argument
Description
DC|AC|TRAN Analysis type for the measurement. If you omit this parameter, HSPICE
defaults to the last analysis mode requested.
result
Name of the measured result in the output.
ERRfun
Error function to use: ERR, ERR1, ERR2, or ERR3.
meas_var
Name of any output variable or parameter in the data command. M
denotes the meas_var in the error equation.
calc_var
Name of the simulated output variable or parameter in the .MEASURE
command to compare with meas_var. C is the calc_var in the error
equation.
MINVAL
If the absolute value of meas_var is less than MINVAL, MINVAL
replaces the meas_var value in the denominator of the ERRfun
expression. Used only in ERR calculation for optimization. Default:
1.0e-12.
IGNOR|YMIN If the absolute value of meas_var is less than the IGNOR value, then
the ERRfun calculation does not consider this point. Default: 1.0e-15.
196
YMAX
If the absolute value of meas_var is greater than the YMAX value, then
the ERRfun calculation does not consider this point. Default: 1.0e+15.
WEIGHT
Calculates error multiplied weight value. Used only in ERR calculation
for optimization. The default is 1.0.
FROM
Specifies the beginning of the ERRfun calculation. For transient
analysis, the FROM value is in units of time. Defaults to the first value
of the sweep variable.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Error Function)
Argument
Description
TO
End of the ERRfun calculation. Default is last value of the sweep
variable.
Description
The relative error function reports the relative difference between two output
variables. You can use this format in optimization and curve-fitting of measured
data. The relative error format specifies the variable to measure and calculate
from the .PARAM variable. To calculate the relative error between the two,
HSPICE uses the ERR, ERR1, ERR2, or ERR3 functions. With this format you
can specify a group of parameters to vary to match the calculated value and the
measured data.
Examples
.measure ac comp1 err1 par(s11m) s11(m)
.measure tran re1 err1 par(out2) v(out) from=1u to=2u
See Also
.OPTION AUTOSTOP (or) .OPTION AUTOST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
197
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE PHASENOISE
.MEASURE PHASENOISE
Enables measurement of phase noise at various frequency points in HSPICE
RF.
Syntax
Find-When ... Phase Noise
.MEASURE PHASENOISE result FIND phnoise At = IFB_value
+ [PRINT 0|1]
.MEASURE PHASENOISE result WHEN phnoise=value [PRINT 0|1]
RMS, average, min, max, and peak-to-peak Phase Noise
.MEASURE PHASENOISE result funcphnoise + [FROM = IFB1] [TO
= IFB2] [PRINT 0|1]
Integral Evaluation of Phase Noise
.MEASURE PHASENOISE result INTEGRAL phnoise + [FROM = IFB1]
[TO = IFB2] [PRINT 0|1]
Derivative Evaluation of Phase noise
.MEASURE PHASENOISE result DERIV[ATIVE] phnoise AT = IFB1
+ [PRINT 0|1]
Amplitude modulation noise
.MEASURE phasenoise result AM[NOISE] phnoise
+ [FROM = IFB1] [TO = IFB2] [PRINT 0|1]
Phase modulation noise
.MEASURE phasenoise result PM[NOISE] phnoise
+ [FROM = IFB1] [TO = IFB2] [PRINT 0|1]
198
Argument
Description
FIND
Selects the FIND function
result
Name of the measured result in the output.
phnoise
.MEASURE PHASENOISE value for phase noise
WHEN
Selects the WHEN function
IFB_value
Input frequency band point value
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE PHASENOISE
Argument
Description
func
Indicates one of the measure command types:
■
■
■
■
■
AVG (average): Calculates the phase noise over the frequency
range.
MAX (maximum): Reports the maximum value of the phase noise
over the specified frequency range.
MIN (minimum): Reports the minimum value of the phase noise over
the specified frequency range.
PP (peak-to-peak): Reports the maximum value, minus the
minimum value of the phase noise over the specified frequency
range.
RMS (root mean squared): Calculates the square root of the phase
noise over the specified frequency range.
FROM...TO
Optional range for input frequency bands (IFB)
INTEGRAL
Integrates the phase noise value from the first to the second IFB
frequency points
DERIVATIVE Finds the derivative of the phase noise at the first IFB frequency point
PM[NOISE]
Measures the phase modulation noise from the specified first to the
second IFB frequency points (when .OPTION PHASENOISEAMPM=1)
AM[NOISE]
Measures the amplitude modulation noise from the specified first to the
second IFB frequency points (when .OPTION PHASENOISEAMPM=1)
Description
This command enables measurement of phase noise at various frequency
points in HSPICE RF.
The .MEASUREPHASENOISE syntax supports yielding the following phase
noise instances in dbc/Hz:
■
Yields the phase noise using FIND or WHEN functions: at a specified input
frequency band (FIND), or phase noise found at a specified input frequency
point (WHEN).
■
Yields the average, RMS, minimum, maximum, or peak-to-peak value of the
phase noise from frequency IFB1 to frequency IFB2, where the value of
func can be RMS, AVG, MIN, MAX or PP. If FROM and TO are not specified,
the value will be calculated over the frequency range specified in the
.PHASENOISE command.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
199
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE PHASENOISE
■
Integrates the phase noise value from the IFB1 frequency to the IFB2
frequency.
■
Finds the derivative of phase noise at the IFB1 frequency point.
Note:
The .MEASURE PHASENOISE command cannot contain an
expression that uses a phase noise variable as an argument. You
also cannot use .MEASUREPHASENOISE for error measurement
and expression evaluation of PHASENOISE.
The HSPICE RF optimization flow can read the measured data from a
.MEASURE PHASENOISE analysis. This flow can be combined in the HSPICE
RF optimization routine with a .MEASUREHBTR analysis.
Examples
Example 1
The FIND keyword yields the result of a variable value at a specific input
frequency band (IFB) point.
.MEASURE PHASENOISE np1 find PHNOISE at=100K
Example 2
The WHEN keyword yields the input frequency point at a specific phase
noise value.
.MEASURE PHASENOISE fcorn1 when PHNOISE=-120
Example 3
The following sample command find functions such as the RMS, AVG,
MIN, MAX, or PP over the frequency range.
.measure PHASENOISE rn1 RMS phnoise
.measure PHASENOISE agn1 AVG phnoise from=100k to=10meg
.measure PHASENOISE nmin MIN phnoise
Example 4
The INTEGRAL command integrates the phase noise across the two
specified Input frequency band points.
.measure PHASENOISE inns1 INTEGRAL phnoise
.measure PHASENOISE rns1 INTEGRAL phnoise from=50k to 500k
Example 5
These DERIV sample commands find the derivative of the phase noise
at one input frequency band point.
.measure PHASENOISE dnf1 DERIVATIVE phnoise at=100k
.measure PHASENOISE fdn1 DERIVATIVE phnoise at=10meg
Example 6
These AM/PM sample commands find the amplitude modulation (AM)
and phase modulation (PM) noise across the specified input frequency
range.
.measure PHASENOISE amp1 AM phnoise from=100k to 400k
.measure PHASENOISE pmp1 PM phnoise from=10meg to=30meg
200
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE PHASENOISE
See Also
.PHASENOISE
.MEASURE PTDNOISE
.MEASURE (FIND and WHEN)
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
.MEASURE (Integral Function)
.MEASURE (Derivative Function)
Measuring Phase Noise with .MEASURE PHASENOISE
.HB
.OPTION PHNOISEAMPM
.OPTION AUTOSTOP (or) .OPTION AUTOST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
201
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE PTDNOISE
.MEASURE PTDNOISE
Allows for the measurement of integrated phase noise, time-point, tdelta-value,
slewrate, and strobed jitter parameters in HSPICE RF.
Syntax
.MEASURE PTDNOISE meas_name STROBEJITTER onoisefreq_sweep
+[PRINT 0|1]
Argument
Description
strobed jitter
Calculated from the noise voltage (integrated over the frequency range
specified by frequency_range), divided by the slewrate at the same
node(s), at the time point specified by time_value. While only
STROBEJITTER can be specified, all of the parameters listed below are
also output to the *.msnptn# file. Unit: sec
integptdnoise Unit: V
timepoint
Unit: sec
tdelta-value
Unit: sec
slewrate
Unit: V/sec
Description
Use to obtain strobed jitter parameters in large signal periodic time-dependent
noise analysis. For more information, see the HSPICE User Guide: RF
Analysis section on Periodic Time-Dependent Noise Analysis (.PTDNOISE).
See Also
.PTDNOISE
.MEASURE Syntax and File Format
202
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Pushout Bisection)
.MEASURE (Pushout Bisection)
Specifies a maximum allowed pushout time to control the distance from failure
in bisection analysis.
Syntax
.MEASURE TRAN result MeasureClause
+ pushout=time [lower|upper] [POSITIVE|NEGATIVE]
+[PRINT 0|1]
-or.MEASURE TRAN result MeasureClause
+ pushout_per=percentage [lower|upper] [POSITIVE|NEGATIVE]
+ [PRINT 0|1]
Argument
Description
result
Name associated with the measured value in the HSPICE output,
can be up to 16 characters long.
pushout=time
The absolute time to obtain the pushout result.
pushout_per=
percentage
Relative error. If you specify a 0.1 relative error, the T_lower or
T_upper and T_pushout have more than a 10% difference in value.
This occurrence causes the iteration to stop and output the
optimized parameter.
lower|upper
Parameter boundary values for pushout comparison. These
arguments are optional. If the parameter is defined as
.PARAM ParamName= OPTxxx(Initial, min, max)
The “lower” means the lower bound “min”, and the “upper” means
the upper bound “max”. The default is lower.
POSITIVE
Pushout constraints only take effect when the measuring results are
larger than the golden measure.
NEGATIVE
Pushout constraints only take effect when the measuring results are
smaller than the golden measure.
Description
Pushout is used only in bisection analysis. In Pushout Bisection, instead of
finding the last point just before failure, you specify a maximum allowed
pushout time to control the distance from failure.
To limit the range you can add both absolute and relative pushout together.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
203
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (Pushout Bisection)
For example:
.Measure Tran pushout When v(D_Output)='vih/2'
+ rise=1 pushout=20p,50p pushout_per=0.1
The final measure result for the preceding example should be in the range of:
| measresult-goldmeas | < Min (pushout_max,
pushout_per*goldmeas)
...or the final measure result should satisfy,
Max(pushout_per*goldmeas, pushout_min)
Examples
Example 1
The parameter to be optimized is Delaytime and the evaluation goal is
setup_prop. The Pushout=1.5n lower means that the setup_prop of the
final solution is not 1.5n far from the setup_prop of the lower bound of the
parameter (0.0n).
.Param DelayTime=Opt1 ( 0.0n, 0.0n , 5.0n )
.Tran 1n 8n Sweep Optimize=Opt1 Result=setup_prop
+ Model=OptMod
.Measure Tran setup_prop Trig v(data)
+ Val='v(Vdd) 2' fall=1 Targ v(D_Output)
+ Val='v(Vdd)' rise=1 pushout=1.5n lower
Example 2
The differences between the setup_prop of the final solution and that of
the lower bound of the parameter (0.0n) is not more than 10%.
.Measure Tran setup_prop Trig v(data)
+ Val='v(Vdd)/2' fall=1 Targ v(D_Output)
+ Val='v(Vdd)' rise=1 pushout_per=0.1 lower
Example 3
Pushout constraints only take effect when the measuring results are
larger than the golden measure.
.MEASURE TRAN result MeasureClause pushout=time
+ pushout_perpercentage POSITIVE
Example 4
Pushout constraints only take effect when the measuring results are
smaller than the golden measure.
.MEASURE TRAN result MeasureClause pushout=time
+ pushout_perpercentage NEGATIVE
See Also
Pushout Bisection Methodology
204
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (ACMATCH)
.MEASURE (ACMATCH)
Introduces special keywords to access results for ACMatch analysis in
HSPICE.
Syntax
.MEASURE AC result [MAX][ACM_Total|ACM_Global|+
ACM_Global(par)|ACM_Local|ACM_Local(dev)] [PRINT 0|1]
Argument
DescriptionDescription
results
Name associated with the measured values in the HSPICE output, can be up
to 16 characters long.
MAX
Sample function; Instead of “MAX” other functions can be used which select
one out of multiple results.
ACM_Total
Output sigma due to global, local, and spatial variations.
ACM_Global
Output sigma due to global variations.
ACM_Global(par) Contribution of parameter (par) to output sigma due to global variations.
ACM_Local
Output sigma due to local variations.
ACM_Local(dev)
Contribution of device (dev) to output sigma due to local variations.
Description
ACMatch analysis saves results using .MEASURE commands, with AC type
(M,P,R,I) for an output variable, as specified on the .ACMatch command. If you
specify multiple output variables the command issues a result for the last one
only. You must specify an AC sweep to produce these kinds of outputs; a single
point sweep is sufficient. ACMatch uses the special keywords shown above to
access the results from the different variation types. For usable keywords with
the .PROBE command, see Output from .PROBE and .MEASURE Commands
for ACMatch in the HSPICE User Guide: Simulation and Analysis.
See Also
.AC
.MEASURE (ACMATCH)
.PROBE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
205
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (DCMATCH)
.MEASURE (DCMATCH)
Introduces special keywords to access the different types of results for
DCMatch analysis in HSPICE.
Syntax
.MEASURE DC result [MAX] [DCM_Total | DCM_global |
+ DCM_Global(par) | DCM_Local | DCM_Local(dev) |
+ DCM_Spatial | DCM_Spatial(par)] [PRINT 0|1]
ArgumentArgume DescriptionDescription
nt
result
Name associated with the measured values in the HSPICE output, can be up
to 16 characters long.
MAX
Sample function. Instead of “MAX,” other functions can be used which select
one out of multiple results.
DCM_Total
Output sigma due to global, local, and spatial variations.
DCM_Global
Output sigma due to global variations.
DCM_Global(par) Contribution of parameter (par) to output sigma due to global variations.
DCM_Local
Output sigma due to local variations.
DCM_Local(dev)
Contribution of device (dev) to output sigma due to local variations.
DCM_Spatial
Output sigma due to local variations.
DCM_Spatial(par) Contribution of parameter (par) to output sigma due to spatial variations.
Description
DCMatch analysis uses special keywords to access the different types of
results. You can save the different results produced by a DCMatch analysis
using the .MEASURE command for the output variable specified on the
.DCMatch command. For keywords to be used with the .PROBE command,
see Syntax for .PROBE Command for DCMatch in the HSPICE User Guide:
Simulation and Analysis. If you specify multiple output variables, the command
produces a result for the last one only. You must specify a DC sweep to
produce these kinds of outputs; a single point sweep is sufficient.
206
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE (DCMATCH)
Examples
In this example, the result systoffset reports the systematic offset of the
amplifier; the result matchoffset reports the variation due to mismatch; and
the result maxoffset reports the maximum (3-sigma) offset of the amplifier.
.MEAS DC systoffset avg V(inp,inn)
.MEAS DC matchoffset avg DCm_local
.MEAS DC maxoffset
param='abs(systoffset)+3.0*matchoffset'
See Also
.DC
.PROBE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
207
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE FFT
.MEASURE FFT
Specifies measurement of FFT results.
Syntax
Syntax #1
.MEASURE FFT result
+ Find [vm|vp|vr|vi|vdb|im|ip|ir|ii|idb](signal) AT=freq
+ [PRINT 0|1]
Syntax #2
.MEASURE FFT result THD signal_name [nbharm=num]
[PRINT 0|1]
Syntax #3
.MEASURE FFT result[SNR|SNDR|ENOB] signal_name
+ [nbharm=num|maxfreq=val] [BINSIZ=num] [PRINT 0|1]
Syntax #4
.MEASURE FFT result SFDR signal_name
+ [minfreq=val][maxfreq=val] [PRINT 0|1]
Argument
Description
result
Name associated with the measured values in the FFT output, can be up
to 16 characters long.
Find
FIND function.
At
Value of the frequency at which the component frequency and signal are
found
frequency
component/signal
Can be any of the following: vm|vp|vr|vi|vdb|im|ip|ir|ii|idb
freq
Specified frequency
THD
Total harmonic distortion
signal_name
User-supplied name of signal
nbharm
Harmonic up to which to carry out the measurement. Default: highest
harmonic in FFT result.
208
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE FFT
Argument
Description
maxfreq
Higher limit of frequency range to carrying out the measurement. Default:
maximum frequency in an FFT result.
minfreq
Lower limit of frequency range to calculate SFDR.
SNR
Signal to noise ratio.
SNDR
Signal to noise-plus-distortion ratio.
ENOB
Effective number of bits.
BINSIZ
Filters out noise component within the bin; the noise component is
calculated from the index of “fundamental_freq_idx+BINSIZ+1”. Default=0.
SFDR
Spurious free dynamic range.
Description
Four syntaxes are provided for finding measurements of several types for FFT
results.
See examples below for sample usage.
■
Syntax #1: Measures a frequency component at certain frequency.
■
Syntax #2: Measures THD of a signal spectrum up to a specified harmonic;
Default: nbharm=maximum harmonic in FFT result
■
Syntax # 3: Measures SNR/SNDR/ENOB of a signal up to a specified
frequency; Defaults: nbharm=maximum harmonic in FFT result;
maxfreq=maximum frequency in FFT result; BINSIZ=0.
■
Syntax # 4: Measures SFDR of a signal from minfreq to maxfreq;
searches the frequency component with maximum magnitude from
minfreq to maxfreq.
An embedded .MEASURE FFT command in a measure file can be called to
perform FFT measurements from previous simulation results as follows:
HSPICE -i *.tr0 -meas measure_file
Examples
Example 1
Measures frequency component at certain frequency.
.meas FFT v12 Find vm(1,2)at=20k
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
209
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE FFT
Example 2
Measures THD of a signal spectrum up to a specified harmonic.
.meas FFT thd56 THD V(node5, node6) nbharm=10
Example 3
Measures SNR/SNDR/ENOB of a signal up to a specified frequency.
.meas FFT snr12 SNDR V(node1, node2) maxfreq=1G
Example 4
Measures SFDR of a signal from minfreq to maxfreq and searching the
frequency component with maximum magnitude from minfreq to
maxfreq.
.meas FFT sfdr9 SFDR V(node9)
Example 5
Filters out the noise component within the bin.
.meas fft snrsrc SNR v(out) BINSIZ=10
See Also
.FFT
Spectrum Analysis
210
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE LSTB
.MEASURE LSTB
Enables the measurement of lstb output variables similar to any other common
ac variable.
Syntax
.MEASURE AC Result FIND LSTB(x) WHEN LSTB(x)=val
.MEASURE AC Result LSTB(x) FROM=val TO=val
Argument
Description
AC
AC analysis result
Result
Result name of an .AC .LSTB analysis
LSTB
Output loop gain as complex numbers
LSTB(x)
■
■
■
■
■
x=DB: Output the dB values of loop gain
x=M: Output magnitude of loop gain
x=P: Output phase of loop gain
x=R: Output real part of loop gain
x=I: Output imaginary part of loop gain
FIND...WHEN
Selects the Find and When functions
FROM...TO
Selects the range of measurement
Description
Use the .MEASURE LSTB statement to measure linear loop stability outputs in
a similar manner to any common ac output variable. Measure phase margin,
gain margin, unity gain frequency, dc gain, etc... from the return ratio waveform
that is generated in the .LSTB analysis. The lstb scalars can be measured as
follows:
.measure lstb out1 gain_margin
.measure lstb out2 phase_margin
.measure lstb out3 unity_gain_freq
.measure lstb out4 loop_gain_minifreq
in which out1 - out4 are names for measured output, lstb is the type name,
and gain_margin, phase_margin, unity_gain_freq, and
loop_gain_minifreq are keywords of scalar variables.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
211
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MEASURE LSTB
Examples
Example 1
Finds the measurement for the output phase of loop gain of phase margin
when the decibel output is 0.
.MEASURE AC PHASE_MARGIN FIND LSTB(P) WHEN LSTB(DB)=0
Example 2
Measures the first output phase of loop gain Integral across a range of 1
to 100k.
.MEASURE AC INTEG1 INTEGRAL LSTB(P) FROM=1k TO=100k
See Also
.LSTB
212
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
.MODEL
Includes an instance of a predefined HSPICE model in an input netlist.
Syntax
Passive and active device model syntax
.MODEL mname type [level=num]
+ [pname1=val1pname2=val2 ...]
See specific element type for supported model parameter information.
Optimization model syntax
.MODEL mname OPT [METHOD=BISECTION|PASSFAIL] [close=num]
+ [max] [cut=val] [difsiz=val] [grad=val] [parmin=val]
+ [relin=val] [relout=val] [absout=val)
+ [itrop=val] [absin=val]
+ [DYNACC=0|1] [cendif=num]
The following syntax is used for a Monte Carlo analysis:
.MODEL mname ModelType ([level=val]
+ [keyword1=val1][keyword2=val2]
+ [keyword3=val3][lot/n/distributionvalue]
+ [DEV/n /distribution value]...)
The following syntax is used for model reliability analysis
.model mname mosra
+ level|mosralevel value
+ [relmodelparam]
Argument
Description
mname
Model name reference. Elements must use this name to refer to the model. If
model names contain periods (.), the automatic model selector might fail. When
used with .MOSRA it is the user-defined MOSFET reliability model name.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
213
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
Argument
Description
type
Model type. Must be one of the following.:
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
level
Model level.
■
■
■
■
■
■
■
214
AMP—operational amplifier model
C—capacitor model
CORE—magnetic core model
D—diode model
L—inductor model or magnetic core mutual inductor model
NJF—n-channel JFET model
NMOS—n-channel MOSFET model
NPN—npn BJT model
OPT—optimization model
PJF—p-channel JFET model
PLOTQ—plot model for the .GRAPH command (obsolete)
PMOS—p-channel MOSFET model
PNP—pnp BJT model
R—resistor model
U—lossy transmission line model (lumped)
W—lossy transmission line model
S—S-parameter
For optimization model, LEVEL=1 specifies the Modified LevenbergMarquardt method. Use this setting with multiple optimization parameters
and goals.
Only Level=1 is available in HSPICE. Additional levels are available in
HSPICE RF. See below This argument is ignored when METHOD has been
specified.
LEVEL=2 (HSPICE RF) specifies the BISECTION method in HSPICE RF.
You would use this setting with one optimization parameter.
LEVEL=3 (HSPICE RF) specifies the PASSFAIL method. You would use this
setting with two optimization parameters.
For transistors, diodes, and some passive element models, see the HSPICE
Reference Manual, Elements and Device Models.
For MOSFET Models, see the HSPICE Reference Manual: MOSFET
Models.
To use custom MOSRA models and for discussion of LEVEL values, refer to
the HSPICE Application Note: Unified Custom Reliability Modeling API
(MOSRA API). Contact your Synopsys technical support team for more
information.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
Argument
Description
pname1 ...
Parameter name. Assign a model parameter name (pname1) from the
parameter names for the appropriate model type. Each model section provides
default values. For legibility, enclose the parameter assignment list in
parentheses and use either blanks or commas to separate each assignment.
Use a plus sign (+) to start a continuation line.
OPT
Keyword to indicate the definition model is for optimization analysis.
METHOD
Specifies an optimization method.
■
METHOD=BISECTION specifies the Bisection method. When the
difference between the two latest test input values is within the error
tolerance and the latest measured value exceeds the goal, bisection has
succeeded and then ends. This process reports the optimized parameter
that corresponded to the test value that satisfies this error tolerance and this
goal (passes).
■
METHOD=PASSFAIL specifies the passfail method. When the difference
between the last two optimization parameter test values is < the error
tolerance and the associated goal measurement fails for one of the values
and passes for the other, bisection has succeeded and then ends. The
process reports the optimization parameter test value associated with the
last passing measurement. “Pass” is defined as a condition in which the
associated goal measurement can produce a valid result. “Fail” is defined as
a condition in which the associated goal measurement is unable to produce
a valid result.
This argument supersedes LEVEL when present.
close
(Optimization) Initial estimate of how close parameter initial value estimates are
to the solution. The close argument multiplies changes in new parameter
estimates. If you use a large close value, the optimizer takes large steps toward
the solution. For a small value, the optimizer takes smaller steps toward the
solution. You can use a smaller value for close parameter estimates and a
larger value for rough initial guesses. The default is 1.0.
■
If close is greater than 100, the steepest descent in the LevenburgMarquardt algorithm dominates.
■
If close is less than 1, the Gauss-Newton method dominates.
For more details, see L. Spruiell, “Optimization Error Surfaces,” Meta-Software
Journal, Volume 1, Number 4, December 1994.
max
(Optimization) Upper limit on close. Use values > 100. The default is 6.0e+5.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
215
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
Argument
Description
cut
(Optimization) Modifies close, depending on how successful iterations are
toward the solution. If the last iteration succeeds, descent toward the close
solution decreases by the cut value. That is, close=close / cut
If the last iteration was not a successful descent to the solution, close increases
by cut squared. That is, close=close * cut * cut.
Cut drives close up or down, depending on the relative success in finding the
solution. The cut value must be > 1. The default is 2.0.
difsiz
(Optimization) Increment change in a parameter value for gradient calculations
(Δx=DIFSIZ ⋅ MAX(x, 0.1) ). If you specify delta in a .PARAM command, then
Δx=delta. The default is 1e-3.
grad
(Optimization) Represents possible convergence if the gradient of the
RESULTS function is less than GRAD. Most applications use values of 1e-6 to
1e-5. Too large a value can stop the optimizer before finding the best solution.
Too small a value requires more iterations. The default is 1.0e-6.
parmin
(Optimization) Allows better control of incremental parameter changes during
error calculations. The default is 0.1. This produces more control over the tradeoff between simulation time and optimization result accuracy. To calculate
parameter increments, HSPICE uses the relationship:
Δpar_val=ΔIFSIZ ⋅ MAX(par_val, PARMIN)
relin
(Optimization) Relative input parameter (delta_par_val / MAX(par_val,1e-6))
for convergence. If all optimizing input parameters vary by no more than RELIN
between iterations, the solution converges. RELIN is a relative variance test so
a value of 0.001 implies that optimizing parameters vary by less than 0.1%from
one iteration to the next. The default is 0.001.
relout
(Optimization) Relative tolerance to finish optimization. For relout=0.001, if the
relative difference in the RESULTS functions from one iteration to the next, is
less than 0.001, then optimization is finished. The default is 0.001.
absout
(Bisection) Absolute tolerance to finish bisection. For absout=0.001, if the
absolute difference in the RESULTS functions from one iteration to the next, is
less than 0.001, then bisection is completed. The default is 0.0, which means
inactive, and use relout.
itropt
(Optimization) Maximum number of iterations. Typically, you need no more than
20-40 iterations to find a solution. Too many iterations can imply that the relin,
grad, or relout values are too small. The default is 20.
216
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
Argument
Description
absin
(Optimization) Overrides relin parameter and ignores relout and itropt; there is
no default value
DYNACC
(Optimization) Dynamic accuracy tolerance setting to accelerate bisection
simulation. The default is 0.
When DYNACC=1, if HSPICE is in accuracy mode, it uses reduced accuracy
simulations to narrow the bisection window, then switches to the original
accuracy algorithm to refine the solution. This method reduces simulation time
by doing the majority of simulations at lower accuracy, which run faster by
taking fewer time steps.
cendif
(Optimization) Point at which more accurate derivatives are desired.
keyword
(Monte Carlo) Model parameter keyword.
distribution
(Monte Carlo) The distribution function name, which must be specified as
GAUSS, AGAUSS, LIMIT, UNIF, or AUNIF. If you do not set the distribution
function, the default distribution function is used. The default distribution
function is uniform distribution.
DEV
(Monte Carlo) DEV tolerance, which is independent (each device varies
independently).
LOT
(Monte Carlo) The LOT tolerance, which requires all devices that refer to the
same model use the same adjustments to the model parameter.
LOT/n
DEV/n
(Monte Carlo) Sets which of ten random number generators numbered 0
through 9 is used to calculate parameter value deviations. This correlates
deviations between parameters in the same model as well as between models.
The generators for DEV and LOT tolerances are distinct: Ten generators exist
for both DEV tracking and LOT tracking. N must be an integer 0 to 9.
mosra
Keyword to indicate the definition model is for MOSRA analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
217
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
Argument
Description
level (alias:
mosralevel)
To use the Synopsys MOSRA model, set LEVEL=1. For compatibility with
HSIM, in the .MODEL statement, 'LEVEL=' can be replaced with
'MOSRALEVEL='. HSPICE will consider them equivalent. Example: The
following two lines will be interpreted the same by HSPICE.
.MODEL my_mod MOSRA LEVEL=1
.MODEL my_mod MOSRA MOSRALEVEL=1
To use custom MOSRA models and for discussion of LEVEL values, refer to the
HSPICE Application Note: Unified Custom Reliability Modeling API (MOSRA
API). Contact your Synopsys technical support team for more information.
RelMode
HSPICE reliability mode level; selects whether a simulation accounts for both
HCI and NBTI effects or either one of them. If the RelMode in the .MOSRA
command is defined as 1 or 2, it takes higher priority and applies to all MOSRA
models. If RelMode in the .MOSRA command is not set or set to 0, then the
RelMode inside individual MOSRA models take precedence for that MOSRA
model only; the rest of the MOSRA models take the RelMode value from
the .MOSRA command. If any other value is set, except 0, 1, or 2, a warning is
issued, and RelMode is automatically set to the default value 0.
■
■
■
0: both HCI and NBTI, Default.
1: HCI only
2: NBTI only
relmodelparam Model parameter for HCI or BTI, when doing a reliability MOSFET device
analysis. See Level 1 MOSRA BTI and HCI Model Parameters in the HSPICE
User Guide: Simulation and Analysis for listing of HCI and NBTI parameters.
Contact Synopsys Technical Support for access to the MOSRA API.
Description
Use this command to include an instance (element) of a predefined HSPICE
model in your input netlist.
For each optimization within a data file, specify a .MODEL command. HSPICE
can then execute more than one optimization per simulation run. The .MODEL
optimization command defines:
■
218
Convergence criteria: (Bisection accuracy is controlled by the parameters:
relin, relout, absin, and itropt. The relin parameter (default 1e-3)
times the bisection window size is the goal accuracy. This goal accuracy is
also influenced by relout (default 1e-3, the difference ratio between last
two iterations) and itropt (default 20 iterations). To keep the same
bisection accuracy, these three parameters need to change accordingly with
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
a changing bisection window size. You can override the relin value by
using the absin option which has no default (see .OPTION ABSIN.) The
absin parameter also ignores itropt and relout.
■
Number of iterations
■
Derivative methods
Examples
Example 1
A standard .model statement.
.MODEL MOD1 NPN BF=50 IS=1E-13 VBF=50 AREA=2 PJ=3 N=1.05
Example 2
Shows the addition of the DYNACC=1 option in an optimization model
card to invoke bisection speedup.
.MODEL optmod OPT METHOD=BISECTION ITROPT=20 dynacc=1 relout=1e20
Example 3
Model command used for a Monte Carlo analysis.
.model m1 nmos level=6 bulk=2 vt=0.7 dev/2 0.1
+ tox=520 lot/gauss 0.3 a1=.5 a2=1.5 cdb=10e-16
+ csb=10e-16 tcv=.0024
Example 4
Transistors M1 through M3 have the same random vto model parameter
for each of the five Monte Carlo runs through the use of the LOT
construct.
...
.model mname nmos level=53 vto=0.4 LOT/agauss 0.1 version=3.22
M1 11 21 31 41 mname W=20u L=0.3u
M2 12 22 32 42 mname W=20u L=0.3u
M3 13 23 33 43 mname W=20u L=0.3u
...
.dc v1 0 vdd 0.1 sweep monte=5
.end
Example 5
Transistors M1 through M3 have different values of the vto model
parameter for each of the Monte Carlo runs through the use of the DEV
construct.
...
.model mname nmos level=54 vto=0.4 DEV/agauss 0.1
M1 11 21 31 41 mname W=20u L=0.3u
M2 12 22 32 42 mname W=20u L=0.3u
M3 13 23 33 43 mname W=20u L=0.3u
...
.dc v1 0 vdd 0.1 sweep monte=5
.end
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
219
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL
Example 6
Establishes a MOS reliability model card.
.model NCH_RA mosra
+ level=1
+ a_hci=1e-2
+ n_hci=1
See Also
Cell Characterization Examples for demo files of .MODEL opt
Method=bisection or passfail
BJT and Diode Examples for all listed *.sp files in the demo group which use
the .MODEL command for npn transistors.
220
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MODEL_INFO
.MODEL_INFO
Enables printout of all or specified MOSFET model parameters for each
simulation.
Syntax
.MODEL_INFO ALL | instance_name1, instance_name2, …,
Argument
Description
ALL
Prints all MOSFET instances.
intance_name1...
instance_name2
Specific MOSFET instance. If the MOSFET instance is in a
.SUBCKT command, it must be written in the full hierarchical
path, e.g.: x1.x2.main.
Description
This command generates a text format file with the suffix *.model_info#.
Note:
If the arguments ALL and instance_name are specified
together, ALL will take higher priority.
Examples
Example 1
Prints all MOSFET instances' model parameters.
.MODEL_INFO ALL
Example 2
Prints the model parameters for devices.
.model_info main x1.m1 x2.m2
Example 3
Prints the model parameters for devices nch.27 and pch.19.
.model_info x_m_11.nch.27 x_m_2.nch.27 x_m_3.pch.19
Example 4
Prints all MOSFET instances' model parameters. (“ALL” takes higher
priority over instances.)
.MODEL_INFO ALL x1.m1
See Also
Using .MODEL_INFO to Print Model Parameters
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
221
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MOSRA
.MOSRA
Starts HSPICE HCI and/or BTI reliability analysis for HSPICE.
Syntax
.MOSRA RelTotalTime=time_value
+ [RelStartTime=time_value] [DEC=value] [LIN=value]
+ [RelStep=time_value] [RelMode=0|1|2] SimMode=[0|1|2|3]
+ [AgingStart=time_value] [AgingStop=time_value]
+ [AgingPeriod=time_value] [AgingWidth=time_value]
+ [AgingInst="inst_name"]
+ [HciThreshold=value] [NbtiThreshold=value]
+ [Integmod=0|1|2] [Xpolatemod=0|1|2]
+ [Tsample1=value] [Tsample2=value]
+ [Agethreshold=value]
+ [MosraLlife=degradation_type_keyword] [DegF=value]
+ [DegFN=value] [DegFP=value]
Argument
Description
RelTotalTime
Final reliability test time to use in post-stress simulation phase. Required
argument.
RelStartTime
Time point of the first post-stress simulation. Default is 0.
DEC
Specifies number of post-stress time points simulated per decade.
LIN
Linear post-stress time points from RelStartTme to RelTotalTime.
RelStep
Post-stress simulation phase on time= RelStep, 2* RelStep, 3* RelStep, …
until it achieves the RelTotalTime; the default is equal to RelTotalTime.
Value is ignored if DEC or LIN value is set.
222
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MOSRA
Argument
Description
RelMode
HSPICE reliability model mode selects whether a simulation accounts for
both HCI and BTI effects or either one of them. If the RelMode in
the .MOSRA command is defined as 1 or 2, it takes higher priority and
applies to all MOSRA models. If RelMode in the .MOSRA command is not
set or set to 0, then the RelMode inside individual MOSRA models take
precedence for that MOSRA model only; the rest of the MOSRA models
take the RelMode value from the .MOSRA command. If any other value is
set, except 0, 1, or 2, a warning is issued, and RelMode is automatically
set to the default value 0.
■
■
■
SimMode
0: both HCI and BTI, Default.
1: HCI only
2: BTI only
■
0: Select pre-stress simulation only
1: Select post-stress simulation only
■
2: Select both pre- and post-stress simulation
■
3: Select continual degradation integration through alters
When SimMode=1
■
■
HSPICE reads in the *.radeg0 file and uses it to update the device
model for reliability analysis; new transient output is generated in a *.tr1
waveform file.
■
The *.radeg file and input netlist must be in the same directory.
■
The netlist stimuli could be different from the SimMode=0 netlist that
generated the *.radeg file.
When SimMode=3
■
■
■
If no .option radegfile is specified in the top level netlist,
simulation will start from fresh device.
If .option radegfile is specified in the top level netlist, HSPICE
reads in the last suite degradation in the radeg file, and continues the
degradation integration and extrapolation from the corresponding circuit
time in the radeg file.
In consecutive alters, the radeg generated from the previous alter run is
read in.
AgingStart
Optionally defines time when HSPICE starts stress effect calculation
during transient simulation. Default is 0.0.
AgingStop
Optionally defines time when HSPICE stops stress effect calculation
during transient simulation. Default is tstop in .TRAN command.
AgingPeriod
Stress period. Scales the total degradation over time.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
223
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MOSRA
Argument
Description
AgingWidth
The AgingWidth (circuit time “on”) argument works with the AgingPeriod
argument. For example: if you specify AgingPeriod=1.0s and
AgingWidth=0.5s, then the circuit is turned on for 0.5s, and turned off for
0.5s. (The period is 1.0s.)
AgingInst
Selects MOSFET devices to which HSPICE applies HCI and/or BTI
analysis. The default is all MOSFET devices with reliability model
appended. The name must be surrounded by quotes. Multiple names
allowed/wildcards supported.
HciThreshold
Optionally, used in post-stress simulation. HCI effect is accounted for in a
particular transistor, based on the specified HCI threshold value. Default is
0.0
NbtiThreshold
Optionally, used in post-stress simulation. BTI effect is accounted for in a
particular transistor, based on this threshold value. Default is 0.0
Integmod
The flag is used to select the integration method and function.
■
■
■
Xpolatemod
0 (default): User-defined integration function in MOSRA API
1: True derivation and integration method
2: Linearized integration method (support non-constant n coefficient)
The flag is used to select the extrapolation method and function.
■
■
■
0 (default): User-defined extrapolation function in MOSRA API
1: Linearization extrapolation method (support non-constant n
coefficient)
2: Two-point fitting extraction and extrapolation method
Tsample1
First simulation time point of stress_total sampling for Xpolatemod=2
Tsample2
Second simulation time point of stress_total sampling for Xpolatemod=2
Agethreshold
Only when the degradation value >= Agethreshold, the MOSFET
information will be printed in the MOSRA output file. Default is 0.
MosraLife
Argument to compute device lifetime calculation for the degradation type
specified. This argument has the same function as .option
mosralife.
DegF
Sets the MOSFET’s failure criteria for lifetime computation. This argument
has the same function as .option degf. If .option degf is specified,
it takes precedence over .mosra degf.
224
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MOSRA
Argument
Description
DegFN
Sets the NMOS's failure criteria for lifetime computation. This argument
has the same function as .option degfn. If .option degfn is
specified, it takes precedence over .mosra degfn.
DegFP
Sets the PMOS's failure criteria for lifetime computation. This argument
has the same function as .option degfp. If .option degfp is
specified, it takes precedence over .mosra degfp.
Description
Use the .MOSRA command to initiate HCI and BTI analysis for the following
models: Level 49, Level 53, Level 54, Level 57, Level 66, Level 69, Level 70,
Level 71, Level 73, and external CMI MOSFET models. This is a two-phase
simulation, the fresh simulation phase and the post stress simulation phase.
During the fresh simulation phase, HSPICE computes the electron age/stress
of selected MOS transistors in the circuit based on circuit behavior and the
HSPICE built-in stress model including HCI and/or BTI effect. During the post
stress simulation phase, HSPICE simulates the degradation effect on circuit
performance, based on the stress information produced during the fresh
simulation phase. If you specify either DEC or LIN, the RelStep value is
ignored.
For a full description refer to the HSPICE User Guide: Simulation and Analysis:
MOSFET Model Reliability Analysis (MOSRA).
Examples
.mosra reltotaltime=6.3e+8 relstep=6.3e+7
+ agingstart=5n agingstop=100n
+ hcithreshold=0 nbtithreshold=0
+ aginginst="x1.*"
See Also
.APPENDMODEL
.MODEL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
225
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MOSRAPRINT
.MOSRAPRINT
Provides .PRINT/.PROBE capability to access the electrical degradation of
the specified element.
Syntax
.MOSRAPRINT output_nameoutput_type(element_name, vds=exp1,
vgs=exp2, vbs=exp3)
Argument
Description
output_name
User-defined output variable; this [email protected]_name is
used as the as output variable name in the output file.
output_type
One of the following output variable types: vth, gm, gds, ids, dids or
dvth
element_name
The element name that the .MOSRAPRINT command applies.
Description
The .MOSRAPRINT command supports the following models: B3SOI, B4SOI,
PSP, BSIM3, BSIM4, HVMOS, HiSIM-HV, and Custom CMI MOSFETS.
This command provides access to device degradation information. The vds,
vgs and vbs are user-specified bias conditions used to characterize the device
electrical property as specified by the output type. There is no order
requirement for vds, vgs, and vbs. Wildcards '?' and '*' are supported in
element_name. The output variable dids reports the change of ids between
post-stress simulation and fresh-simulation. dvth reports the percentage
change of vth between post-stress simulation and fresh-simulation. The output
file format is the same as the measurement file format with file extension *.ra.
.MOSRAPRINT does approximate calculation to get the ids.
Examples
The following syntax prints the ids value of the MOSFET m1, when vds =
5vgs=5, vbs=0, at each reltime point.
.MOSRA reltotaltime=5e+7 relstep=1e+7
.MOSRAPRINT ids(m1, vds=5, vgs=5, vbs=0)
See Also
.MOSRA
226
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.MOSRA_SUBCKT_PIN_VOLT
.MOSRA_SUBCKT_PIN_VOLT
When a MOSFET is wrapped by a subckt-based macro model, this command
specifies the subckt terminal voltages used by MOSRA model evaluation.
Syntax
.MOSRA_SUBCKT_PIN_VOLT subckt=subckt_name1,
+ subckt_name2,...
Description
Use this command to specify subckt-based macro terminal voltages HSPICE
will use for MOSRA model evaluation.
subckt: The subcircuit name whose terminal voltages to be used for MOSRA
model evaluation.
Note:
There is a limitation to this capability. The subckt-based macro
model can contain only one MOSFET, and the number and
definition of subckt terminals must be consistent with HSPICE
MOSFET terminal number and definition.
Examples
In this example, HSPICE will use subckt sub1's terminal voltages v(d)/v(g)/
v(s)/v(b) , instead of the MOSFET M1's terminal voltages, v(d1)/v(g1)/v(s1)/
v(b1), v(d1)/v(g1)/v(s1)/v(b) for MOSRA model evaluation.
.subckt sub1 d g s b ...
M1 d1 g1 s1 b ...
Rd d d1 1k
Rs s s1 1k
Rg g g1 1k
.model ...
.ends
.mosra_subckt_pin_volt subckt=sub1
...
.end
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
227
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.NODESET
.NODESET
Initializes specified nodal voltages for DC operating point analysis and corrects
convergence problems in DC analysis.
Syntax
.NODESET V(node1)=val1 V(node2)=val2 ... [subckt=sub_name]
-or.NODESET node1val1node2val2 [subckt=sub_name]
Argument
Description
node1 ...
Node numbers or names can include full paths or circuit numbers.
val1
Voltages.
subckt=sub_ Initial condition is set to the specified node name(s) within all instances
name
of the specified subcircuit name. This subckt setting is equivalent to
placing the .NODESET command within the subcircuit definition.
Description
Use the .NODESET command to set a seed value for the iterative DC
convergence algorithm for all specified nodal voltages. Use this to correct
convergence problems in DC analysis. How it behaves depends on whether the
.TRAN analysis command includes the UIC parameter.
Forcing circuits are connected to the .NODESET nodes for the first iteration of
DC convergence. To increase the number of held iterations, see .OPTION
DCHOLD. The forcing circuits are then removed and Newton Raphson
iterations continued until DC convergence is obtained. The .NODESET nodes
can move to their true DC operating points. For this reason, .NODESET should
be used to provide initial guesses to either speed up convergence, aid nonconvergence, or to set the preferred DC state of multi-stable nodes. If the DC
operating voltage of a .NODESET node is appreciably different than the voltage
in the .NODESET command you should investigate the circuit to determine why.
It is a likely error condition.
Note:
In nearly all applications you should use .NODESET to ensure a
true DC operating point. Set intentionally floating (or very high
impedance) nodes to a known good voltage using .IC.
If you do not specify the UIC parameter in the .TRAN command then use
.NODESET to set seed values for an initial guess for DC operating point
228
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.NODESET
analysis. If the node value is close to the DC solution then you will enhance
convergence of the simulation.
If you specify the UIC parameter in the .TRAN command, HSPICE does not
calculate the initial DC operating point, but directly enters transient analysis.
When you use .TRAN UIC, the .TRAN node values (at time zero) are
determined by searching for the first value found in this order: from .IC value,
then IC parameter on an element command, then .NODESET value, otherwise
use a voltage of zero.
Note that forcing a node value of the DC operating point might not satisfy KVL
and KCL. In this event you might see activity during the initial part of the
simulation. This might happen if you use UIC and do not specify some node
values, when you specify too many conflicting .IC values, or when you force
node values and topology changes. Forcing a node voltage applies a fixed
equivalent voltage source during DC analysis and transient analysis removes
the voltage sources to calculate the second and later time points.Therefore to
correct DC convergence problems use .NODESETs (without .TRAN UIC)
liberally (when a good guess can be provided) and use .ICs sparingly (when
the exact node voltage is known).
In addition, you can use wildcards in the .NODESET command. See Using
Wildcards on Node Names in the HSPICE User Guide: Simulation and
Analysis.
Examples
Example 1
.NODESET V(5:SETX)=3.5V V(X1.X2.VINT)=1V
.NODESET V(12)=4.5 V(4)=2.23
.NODESET 12 4.5 4 2.23 1 1
Example 2
All setings in this statement are applied to subckt my_ff.
.NODESET V(in)=0.9 subckt=my_ff
See Also
.DC
.IC
.OPTION DCHOLD
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
229
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.NOISE
.NOISE
Controls the noise analysis of the circuit.
Syntax
.NOISE v(out) vin [interval|inter=x]
+ [listckt=[1|0]]
+ [listfreq=frequencies|none|all]
+ [listcount=num] [listfloor=val]
+ [listsources=1|0|yes|no]]
Argument
Description
v(out)
Nodal voltage or branch current output variable. Defines the node or branch
at which HSPICE sums the noise.
vin
Independent voltage source to use as the noise input reference
interval | inter
Interval at which HSPICE prints a noise analysis summary. inter specifies
how many frequency points to summarize in the AC sweep. If you omit
inter or set it to zero, HSPICE or HSPICE RF does not print a summary. If
inter is equal to or greater than one, HSPICE prints summary for the first
frequency, and once for each subsequent increment of the interval
frequency. The noise report is sorted according to the contribution of each
node to the overall noise level. If any of the LIST* arguments below are
specified, the output information will follow the format required by LIST*,
and interval does not influence the output information for later sweeps.
listckt= [1|0]
■
■
230
1: The contribution of each subcircuit is listed in the .lis file and you can
view the subcircuit noise contribution curve in WaveView.
0: (default) HSPICE does not list the noise contribution of any subcircuits.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.NOISE
Argument
Description
listfreq=
(none|all|freq1
freq2....)
Dumps the element noise figure value to the .lis file. You can specify which
frequencies the element phase noise value dumps. The frequencies must
match the sweep_frequency values defined in the parameter_sweep,
otherwise they are ignored. In the element phase noise output, the elements
that contribute the largest phase noise are dumped first. The frequency
values can be specified with the NONE or ALL keyword, which either dumps
no frequencies or every frequency defined in the parameter_sweep.
■
ALL: output all of the frequency points (default, if LIST* is required.)
NONE: do not output any of the frequency points
■
freq1 freq2...: output the information on the specified frequency points
Frequency values must be enclosed in parentheses. For example:
listfreq=(none)listfreq=(all)listfreq=(1.0G)listfreq=(1
.0G, 2.0G)
■
listcount=num
Outputs the first few noise elements that make the biggest contribution to NF.
The number is specified by num. The default is to output all of the noise
element contribution to NF. The NF contribution is calculated with the source
impedance equal to the Zo of the first port.
listfloor=val
Contribution to the output noise power greater than the value specified by
LISTFLOOR. Default is to output all the noise elements. The unit of
LISTFLOOR is V2/hz
listsources=
[1|0|yes|no]
Defines whether or not to output the contribution of each noise source of
each noise element. Default is no/0.
Description
Use this command and .AC commands to control the noise analysis of the
circuit. You can use this command only with an .AC command. Noise
contributor tables are generated for every frequency point and every circuit
device. The last four arguments allow users to better control the output
information.
Examples
Example 1
This example sums the output noise voltage at the node 5 by using the
voltage source VIN as the noise input reference and prints a noise
analysis summary every 10 frequency points.
.NOISE V(5) VIN 10
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
231
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.NOISE
Example 2
Sums the output noise current at the r2 branch by using the voltage
source VIN as the noise input reference and prints a noise analysis
summary every 5 frequency points.
.NOISE I(r2) VIN 5
Example 3
Shows the list subcircuit option turned on and sample results:
***************************************************************
subcircuit squared noise voltages (sq v/hz)
x1 total 1.90546e-20
x7 total 7.14403e-19
x1.x3 total 1.90546e-20
***************************************************************
See Also
.AC
232
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.OP
.OP
Calculates the DC operating point of the circuit; saves circuit voltages at
multiple timesteps.
Syntax
.OP format time format time... [interpolation]
...
.op voltage time1 time2...
Argument
Description
format
Any of the following keywords. Only the first letter is required. The default is ALL
■
ALL: Full operating point, including voltage, currents, conductances, and
capacitances. This parameter outputs voltage/current for the specified time.
■
BRIEF: One-line summary of each element’s voltage, current, and power.
Current is stated in milliamperes and power in milliwatts.
■
CURRENT: Voltage table with a brief summary of element currents and power.
■
DEBUG: Usually invoked only if a simulation does not converge. Debug prints
the non-convergent nodes with the new voltage, old voltage, and the tolerance
(degree of non-convergence). It also prints the non-convergent elements with
their tolerance values.
■
NONE: Inhibits node and element printouts, but performs additional analysis
that you specify.
■
VOLTAGE: Voltage table only.
The preceding keywords are mutually-exclusive; use only one at a time.
time
Time at which HSPICE prints the report. HSPICE RF returns node voltages only
if time (t) is 0.
interpolation Interpolation method for .OP time points during transient analysis or no
interpolation. Only the first character is required; that is, typing i has the same
effect as typing interpolation. Default is not active.If you specify interpolation, all
of the time points in the .OP command (except time=0) use the interpolation
method to calculate the OP value during the transient analysis. If you use this
keyword, it must be at the end of the .OP command. HSPICE ignores any word
after this keyword.
Description
Use this command to calculate the DC operating point of the circuit. You can
also use the .OP command to produce an operating point during a transient
analysis. You can include only one .OP command in a simulation.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
233
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.OP
If an analysis requires calculating an operating point you do not need to specify
the .OP command; HSPICE calculates an operating point. If you use a .OP
command and if you include the UIC parameter in a .TRAN analysis command,
then simulation omits the time=0 operating point analysis and issues a
warning in the output listing.
Use .OP to output circuit node voltages at different timesteps to *.ic0 files. You
can replace use of the .SAVE command to save node voltages. The *.ic0 files
are identical to those created by the .SAVE command. (Remove.SAVE
commands to avoid conflict with the .OP command used to save node
voltages.)
If you want to generate *.dp# files for your transient simulations, use .OPTION
OPFILE in your netlist.
Note:
Without .OP in the netlist, HSPICE does not create an *.op0 file.
Operating point information is printed in *.lis, *op0 and psf format
files. HICUM level 0 information is also supported.
Examples
Example 1 calculates:
■
Operating point at .5ns.
■
Currents at 10 ns for the transient analysis.
■
Voltages at 17.5 ns, 20 ns and 25 ns for the transient analysis.
Example 1
.OP .5NS CUR 10NS VOL 17.5NS 20NS 25NS
Example 2 calculates a complete DC operating point solution.
Example 2
.OP
See Also
.TRAN
.OPTION OPFILE
234
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.OPTION (or) .OPTIONS
.OPTION (or) .OPTIONS
Modifies various aspects of an HSPICE simulation; individual options for
HSPICE and HSPICE RF commands are described in Chapter 3, HSPICE and
RF Netlist Simulation Control Options.
Syntax
.OPTION opt1 [opt2opt3 ...]
Argument
Description
opt1 ...
Input control options. Many options are in the form opt=x, where opt is the
option name and x is the value assigned to that option.
Description
Use this command to modify various aspects of an HSPICE simulation,
including:
■
output types
■
accuracy
■
speed
■
convergence
You can set any number of options in one .OPTION command, and you can
include any number of .OPTION commands in an input netlist file. Most options
default to 0 (OFF) when you do not assign a value by using
either .OPTIONopt=valor the option with no assignment: .OPTIONopt.
To reset options, set them to 0 (.OPTIONopt=0). To redefine an option, enter a
new .OPTION command; HSPICE uses the last definition.
You can use the following types of options with this command. For detailed
information on individual options, see Chapter 3, HSPICE and RF Netlist
Simulation Control Options.
■
General Control Options
■
Input/Output Controls
■
Model and Variation Definition
■
Analysis
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
235
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.OPTION (or) .OPTIONS
For instructions on how to use options that are relevant to a specific simulation
type, see the appropriate analysis chapters in the HSPICE User Guide:
Simulation and Analysis for:
■
Initializing DC-Operating Point Analysis
■
Pole-Zero Analysis
■
Spectrum Analysis
■
Transient Analysis
■
AC Small-Signal and Noise Analysis
■
Linear Network Parameter Analysis
■
Timing Analysis Using Bisection
■
Monte Carlo - Traditional Flow and Statistical Analysis
■
Analyzing Variability and Using the Variation Block
■
Monte Carlo Analysis Variation Block Flow
■
Mismatch Analyses
■
Optimization
■
RC Reduction and Post-Layout Simulation
■
MOSFET Model Reliability Analysis (MOSRA)
Examples
.OPTION BRIEF $ Sets BRIEF to 1 (turns it on)
* Netlist, models,
...
.OPTION BRIEF=0 $ Turns BRIEF off
This example sets the BRIEF option to 1 to suppress a printout. It then resets
BRIEF to 0 later in the input file to resume the printout.
236
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PARAM (or) .PARAMETER (or) .PARAMETERS
.PARAM (or) .PARAMETER (or) .PARAMETERS
Defines parameters in HSPICE and HSPICE RF.
Syntax
Simple parameter assignment:
.PARAM ParamName=RealNumber
Algebraic parameter assignments:
.PARAM ParamName=’AlgebraicExpression’
.PARAM ParamName1=ParamName2
User-defined functions:
.PARAM ParamName(pv1[pv2])=’Expression’
Redefined analysis functions—Variability definitions (see .PARAM Distribution
Function:
.PARAM ParamName=DistributionFunction(Arguments)
Optimization parameter assignment:
.PARAM ParamName=OPTxxx (initial_guess, low_limit,
+ upper_limit)
.PARAM ParamName=OPTxxx (initial_guess, low_limit,
+ upper_limit, delta)
String parameter assignment:
.PARAM ParamName=str('string')
Argument
Description
parameter
Parameter to vary.
■
Initial value estimate.
Lower limit.
■
Upper limit.
If the optimizer does not find the best solution within these constraints, it attempts
to find the best solution without constraints.
■
OPTxxx
Optimization parameter reference name. The associated optimization analysis
references this name. Must agree with the OPTxxx name in the analysis command
associated with an OPTIMIZE keyname.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
237
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PARAM (or) .PARAMETER (or) .PARAMETERS
Argument
Description
delta
The final parameter value is the initial guess ± (n⋅ delta). If you do not specify delta,
the final parameter value is between low_limit and upper_limit. For example, you
can use this parameter to optimize transistor drawn widths and lengths, which must
be quantized.
Description
Use this command to define parameters. Parameters in HSPICE are names
that have associated numeric values.
Note:
A .PARAM statement with no definition is illegal.
A parameter definition always uses the last value found in the input netlist
(subject to global parameter rules).
Use any of the following methods to define parameters:
■
A simple parameter assignment is a constant real number. The parameter
keeps this value unless a later definition changes its value or an algebraic
expression assigns a new value during simulation. HSPICE does not warn
you if it reassigns a parameter.
■
An algebraic parameter (equation) is an algebraic expression of real values,
a predefined or user-defined function or circuit or model values. Enclose a
complex expression in single quotes to invoke the algebraic processor,
unless the expression begins with an alphabetic character and contains no
spaces. A simple expression consists of a single parameter name. To use
an algebraic expression as an output variable in a .PRINT, or .PROBE
command, use the PARAM keyword.
■
A user-defined function assignment is similar to an algebraic parameter.
HSPICE extends the algebraic parameter definition to include function
parameters, used in the algebraic that defines the function. You can nest
user-defined functions up to three levels deep.
■
A predefined analysis function. HSPICE provides several specialized
analysis types, which require a way to control the analysis:
•
Temperature functions (fn)
•
Optimization guess/range
HSPICE also supports the following predefined parameter types:
■
238
Frequency
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PARAM (or) .PARAMETER (or) .PARAMETERS
■
Time
■
Monte Carlo functions
Note:
To print the final evaluated values of all .PARAM commands in the
netlist, use .OPTION LIST. This helps you avoid seeing the
same value for every time point if you run a transient analysis.
Examples
Example 1
Examples 1-3 illustrate predefined analysis function
.PARAM mcVar=Agauss(1.0,0.1,1)
Example 2
In this example, uox and vtx are the variable model parameters, which
optimize a model for a selected set of electrical specifications. The
estimated initial value for the vtx parameter is 0.7 volts. You can vary this
value within the limits of 0.3 and 1.0 volts for the optimization procedure.
The optimization parameter reference name (OPT1) references the
associated optimization analysis command (not shown).
PARAM vtx=OPT1(.7,.3,1.0) uox=OPT1(650,400,900)
Example 3
.PARAM fltmod=str('bpfmodel')
s1 n1 n2 n3 n_ref fqmodel=fltmod zo=50 fbase=25e6 fmax=1e9
Example 4
Simple parameter assignment
.PARAM power_cylces=256
Example 5
Numerical parameter assignment
.PARAM TermValue=1g
rTerm Bit0 0 TermValue
rTerm Bit1 0 TermValue
...
Example 6
Parameter assignment using expressions
.PARAM Pi
=’355/113’
.PARAM Pi2
=’2*Pi’
.PARAM npRatio
=2.1
.PARAM nWidth
=3u
.PARAM pWidth
=’nWidth * npRatio’
Mp1
... <pModelName> W=pWidth
Mn1
... <nModelName> W=nWidth
...
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
239
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PARAM (or) .PARAMETER (or) .PARAMETERS
Example 7
Algebraic parameter
.param x=cos(2)+sin(2)
Example 8
Algebraic expression as an output variable
.PRINT DC v(3) gain=PAR(‘v(3)/v(2)’)
+ PAR(‘V(4)/V(2)’)
Example 9
User-defined functions
.PARAM MyFunc( x, y )=‘Sqrt((x*x)+(y*y))’
.PARAM CentToFar (c)
=’(((c*9)/5)+32)’
.PARAM F(p1,p2)
=’Log(Cos(p1)*Sin(p2))’
.PARAM SqrdProd (a,b)
=’(a*a)*(b*b)’
Example 10 Undefined .PARAM statement results in a warning requesting parameter
variables with their respective values or expressions.
.PARAM $ Illegal as a standalone netlist command.
See Also
.OPTION LIST
240
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PAT
.PAT
Specifies predefined pattern names to be used in a pattern source; also
defines new patnames.
Syntax
.PAT PatName=data [RB=val][R=int]
.PAT patName=[component 1... component n] [RB=val]
+ [R=repeat]
[or]
.PAT PatName=data [RB=param_expr1] [R=param_expr2]
.PAT patName=[component 1 ... component n] [RB=param_expr1]
+ [R=param_expr2]
Argument
Description
data
String of 1, 0, M, or Z that represents a pattern source. The first letter
must be B to represent it as a binary bit stream. This series is called
b-string. A 1 represents the high voltage or current value, and a 0 is
the low voltage or current value. An M represents the value that is
equal to 0.5*(vhi+vlo), and a Z represents the high impedance state
(only for voltage source).
PatName
Pattern name that has an associated b-string or nested structure.
component
Elements that make up a nested structure. Components can be bstrings or a patname defined in other .PAT commands.
RB=val
Starting component of a repetition. The repeat data starts from the
component or bit indicated by RB. RB must be an integer. If RB is
larger than the length of the NS or b-string, an error is issued. If it is
less than 1, it is automatically set to 1.
R=repeat
Specifies how many times the repeating operation is executed. With
no argument, the source repeats from the beginning of the nested
structure or b-string. If R=-1, the repeating operation continues
infinitely. The R must be an integer. If it is less than -1, it is
automatically set to 0.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
241
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PAT
Description
When the .PAT command is used in an input file, some patnames are
predefined and can be used in a pattern source. Patnames can associate a bstring or nested structure, two different types of pattern sources. In this case, a
b-string is a series of 1, 0, m, and z states. The nested structure is a
combination of a b-string and another netlisted structure defined in the .PAT
command. The .PAT command can also be used to define a new patname,
which can be a b-string or nested structure.
Avoid using a predefined patname to define another patname to lessen the
occurrence of a circular definition for which HSPICE issues an error report.
Nested structures must use brackets “[ ]”, but HSPICE does not support using
multiple brackets in one command. If you need to use another nested structure
as a component, define it in a new .PAT command.
Examples
Example 1
Shows eight instances of the .PAT command used for a b-string.
.PAT a1=b1010 r=1 rb=1
.PAT a1=b10101010
.PAT a1=b1010 b0011 r=1 rb=2
.PAT a1=b1010 b0011011
.PAT a1=b1010 r=1 rb=1 b0011 r=1 rb=2
.PAT a1=b10101010 b0011011
.PAT a1=b1010 b0011 r=2 rb=2
.PAT a1=b1010 b0011011011
Example 2
.PAT
.PAT
.PAT
.PAT
Shows four instances of how an existing patname is used to define a new
patname:
a1=b1010 r=1 rb=1
a2=a1
a1=b1010 r=1 rb=1
a2=b1010 r=1 rb=1
Example 3
Shows a nested structure:
.PAT a1=[b1010 r=1 rb=2 b1100]
242
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PAT
Example 4
Shows several instances of how a predefined nested structure is used as
a component in a new nested structure:
.PAT a1=[b1010 r=1 rb=2 b1100] r=1 rb=1
.PAT a2=[a1 b0m0m] r=2 rb=1
.PAT a1=[b1010 r=1 rb=2 b1100] r=1 rb=1
.PAT a2=a1 b0m0m a1 b0m0m a1 b0m0m
.PAT a1=b1010 r=1 rb=2 b1100 b1010 r=1 rb=2 b1100
.PAT a2=b1010 r=1 rb=2 b1100 b1010 r=1 rb=2 b1100 b0m0m
+ b1010 r=1 rb=2 b1100 b1010 r=1 rb=2 b1100 b0m0m
+ b1010 r=1 rb=2 b1100 b1010 r=1 rb=2 b1100 b0m0m
Example 5
.PAT
.PAT
.PAT
.PAT
.PAT
.PAT
Shows several instances of how a predefined nested structure is used as
a component in a new nested structure:
a1=[b1010 r=1 rb=2 b1100] r=1 rb=2
a2=[a1 b0m0m] r=2 rb=2
a1=[b1010 r=1 rb=2 b1100] r=1 rb=2
a2=a1 b0m0m b0m0m b0m0m
a1=b1010 r=1 rb=2 b1100 b1100
a2=b1010 r=1 rb=2 b1100 b1100 b0m0m b0m0m b0m0m
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
243
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PHASENOISE
.PHASENOISE
Performs phase noise analysis on autonomous (oscillator) circuits in HSPICE
RF.
Syntax
.PHASENOISE outputfrequency_sweep [method=0|1|2]
+ [carrierindex=int] [listfreq=(frequencies|none|all)]
+ [listcount=val] [listfloor=val] [listsources=on|off]
+ [spurious=0|1]
Argument
Description
output
Output node, pair of nodes, or 2-terminal element. HSPICE RF
references phase noise calculations to this node (or pair of nodes).
Specify a pair of nodes as V(n+,n-). If you specify only one node,
V(n+), then HSPICE RF assumes that the second node is ground.
You can also specify a 2-terminal element.
frequency_sweep Sweep of type LIN, OCT, DEC, POI, or SWEEPBLOCK. Specify the
type, nsteps, and start and stop time for each sweep type, where:
■
type = Frequency sweep type, such as OCT, DEC, or LIN.
nsteps = Number of steps per decade or total number of steps.
■
start = Starting frequency.
■
stop = Ending frequency.
The four parameters determine the offset frequency sweep about
the carrier used for the phase noise analysis.
■
■
■
■
■
■
METHOD
244
LIN type nsteps start stop
OCT type nsteps start stop
DEC type nsteps start stop
POI type nsteps start stop
SWEEPBLOCK freq1 freq2 ... freqn
■
METHOD=0 (default) selects the Nonlinear Perturbation (NLP)
algorithm, which is used for low-offset frequencies.
■
METHOD=1 selects the Periodic AC (PAC) algorithm, which is
used for high-offset frequencies.
■
METHOD=2 selects the Broadband Phase Noise (BPN)
algorithm, which you can use to span low and high offset
frequencies.
You can use METHOD to specify any single method.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PHASENOISE
Argument
Description
carrierindex
Harmonic index of the carrier at which HSPICE RF computes the
phase noise (optional). The phase noise output is normalized to
this carrier harmonic. The default is 1.
listfreq
Element phase noise value written to the .lis file. You can specify
which frequencies the element phase noise value dumps. The
frequencies must match the sweep_frequency values defined in the
parameter_sweep, otherwise they are ignored.In the element
phase noise output, the elements that contribute the largest phase
noise are dumped first. The frequency values can be specified with
the NONE or ALL keyword, which either dumps no frequencies or
every frequency defined in the parameter_sweep. Frequency
values must be enclosed in parentheses. For
example:listfreq=(none)listfreq=(all)listfreq=(1.0G)listfreq=(1.0G,
2.0G)The default value is the first frequency value.
listcount
Dumps the element phase noise value to the .lis file, which is
sorted from the largest to smallest value. You do not need to dump
every noise element; instead, you can define listcount to dump the
number of element phase-noise frequencies. For example,
listcount=5 means that only the top 5 noise contributors are
dumped. The default value is 20.
listfloor
Dumps the element phase noise value to the .lis file and defines a
minimum meaningful noise value (in dBc/Hz units). Only those
elements with phase-noise values larger than the listfloor value are
dumped. For example, listfloor=-200 means that all noise values
below -200 (dbc/Hz) are not dumped. The default value is -300 dbc/
Hz.
listsources
Writes the element phase-noise value to the .lis file. When the
element has multiple noise sources, such as a level 54 MOSFET,
which contains the thermal, shot, and 1/f noise sources. When
dumping the element phase-noise value you can decide if you need
to dump the contribution from each noise source. You can specify
either ON or OFF: ON dumps the contribution from each noise
source and OFF does not. The default value is OFF.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
245
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PHASENOISE
Argument
Description
spurious
Additional .HBAC analysis that predicts the spurious contributions
to the phase noise. Spurs result from deterministic signals present
within the circuit. In most cases, the spurs are very small signals
and do not interfere with the steady-state operation of the oscillator
but do add energy to the output spectrum of the oscillator. The
energy that the spurs adds might need to be included in jitter
measurements. 0 - No spurious analysis (default)1 - Initiates a
spurious noise analysis
Description
Use this command to invoke phase noise analysis on autonomous (oscillator)
circuits.
See Also
.HB
.HBAC
.HBOSC
.SN
.SNAC
.SNOSC
.PRINT
.PROBE
Identifying Phase Noise Spurious Signals
246
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PKG
.PKG
Provides the IBIS Package Model feature; automatically creates a series of Welements or discrete R, L and C components.
Syntax
.PKG pkgname
+ file = ’pkgfilename’
+ model = ’pkgmodelname’
Argument
Description
pkgname
Package card name
pkgfilename
Name of a .pkg or .ibs file that contains package models.
pkgmodelname
Working model in the .pkg file
Description
The .PKG command provides the IBIS Package Model feature. It supports both
sections and matrixes.
The .PKG command automatically creates a series of W-elements or discrete
R, L and C components. The following nodes are referenced in the netlist:
■
Nodes on the die side:
’pkgname’_’pinname’_dia
■
Nodes on the pin side:
’pkgname’_’pinname’
See Example 2 for how pin1 is referenced.
■
If package = 0 in the .IBIS card, then no package information is added.
■
If package = 1 or 2, then the package information in the .ibs file is added.
■
If package = 3, then the package information in the .pkg file is added.
Examples
Example 1
Illustrates a typical .PKG statement.
.pkg p_test
+ file=’processor_clk_ff.ibs’
+ model=’FCPGA_FF_PKG’
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
247
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PKG
Example 2
Shows how pin1 is referenced.
p_test_pin1_dia and p_test_pin1
Example 3
The element name becomes:
w_p_test_pin1_? ? or r_p_test_pin1_? ? ...
See Also
.EBD
.IBIS
248
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.POWER
.POWER
Prints a table containing the AVG, RMS, MAX, and MIN measurements for
specified signals in HSPICE RF.
Syntax
.POWER signal [REF=vname FROM=start_time TO=end_time]
Argument
Description
signal
Signal name.
vname
Reference name.
start_time Start time of power analysis period. You can also use parameters to define
time.
end_time
End time of power analysis period. You can also use parameters to define
time.
Description
Use this command to print a table containing the AVG, RMS, MAX, and MIN
measurements for every signal specified.
By default, the scope of these measurements are set from 0 to the maximum
timepoint specified in the .TRAN command.
For additional information, see POWER Analysis in the HSPICE User Guide:
RF Analysis.
Examples
Example 1
No simulation start and stop time is specified for the x1.in signal, so the
simulation scope for this signal runs from the start (0ps) to the last .tran
time (100ps).
.power x1.in
.tran 4ps 100ps
Example 2 shows how you can use the FROM and TO times to specify a
separate measurement start and stop time for each signal. In this example.
■
The scope for simulating the x2.in signal is from 20ps to 80ps.
■
The scope for simulating the x0.in signal is from 30ps to 70ps.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
249
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.POWER
Example 2
.param myendtime=80ps
.power x2.in REF=a123 from=20ps to=80ps
.power x0.in REF=abc from=30ps to=’myendtime - 10ps’
See Also
.TRAN
.OPTION SIM_POWER_ANALYSIS
.OPTION SIM_POWER_TOP
.OPTION SIM_POWERPOST
.OPTION SIM_POWERSTART
.OPTION SIM_POWERSTOP
250
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.POWERDC
.POWERDC
Calculates the DC leakage current in the design hierarchy.
Syntax
.POWERDC keywordsubckt_name1...
Argument
Description
keyword
One of these keywords:
■
■
subckt_name#
TOP – prints the power for top-level instances
ALL (default) – prints the power for all instances
Prints the power of all instances in this subcircuit definition
Description
Use this command to calculate the DC leakage current in the design hierarchy.
This option prints a table containing the measurements for AVG, MAX, and MIN
values for the current of every instance in the subcircuit. This table also lists the
sum of the power of each port in the subcircuit.
For additional information, see POWER Analysis in the HSPICE User Guide:
RF Analysis.
You can use the SIM_POWERDC_HSPICE and SIM_POWERDC_ACCURACY
options to increase the accuracy of the .POWERDC command.
See Also
.OPTION SIM_POWERDC_ACCURACY
.OPTION SIM_POWERDC_HSPICE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
251
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PRINT
.PRINT
Prints the values of specified output variables.
Syntax
.PRINT antype ov1 [ov2 ... ]
Argument
Description
antype
Type of analysis for outputs. Can be one of the following types:
DC, AC, TRAN, NOISE, or DISTO.
ov1 ...
Output variables to print. These are voltage, current, or element template
variables from a DC, AC, TRAN, NOISE, or DISTO analysis.
Description
Use this command to print the values of specified output variables. You can
include wildcards in .PRINT commands. You can also use the iall keyword
in a .PRINT command to print all branch currents of all diode, BJT, JFET, or
MOSFET elements in your circuit design. By default, the .PRINT command
prints out simulation data at a time interval of tstep of .TRAN command, so the
number of points for this output data reported in the *.lis are the “# points”
shown at the end of *.lis file.
Examples
Example 1
Three cases of invoking the print function:
In Case 1, if you replace the .PRINT command with: .print TRAN
v(din)i(mnx), then all three cases have identical .sw0 and .tr0 files.
If you replace the .printcommand with: .print DC v(din) i(mnx), then
the .sw0 and .tr0 files are different.
* CASE 1
.print v(din) i(mxn18)
.dc vdin 0 5.0 0.05
.tran 1ns 60ns
* CASE 2
.dc vdin 0 5.0 0.05
.tran 1ns 60ns
.print v(din) i(mxn18)
* CASE 3
.dc vdin 0 5.0 0.05
.print v(din) i(mxn18)
.tran 1ns 60ns
252
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PRINT
Example 2
Example 2 prints the results of a transient analysis for the nodal voltage
named 4. It also prints the current through the voltage source named VIN.
It also prints the ratio of the nodal voltage at the OUT and IN nodes.
.PRINT TRAN V (4) I(VIN) PAR(`V(OUT)/V(IN)')
Example 3
In Example 3:
Depending on the value of the ACOUT option, VM(4,2) prints the AC
magnitude of the voltage difference, or the difference of the voltage
magnitudes between nodes 4 and 2.
VR(7) prints the real part of the AC voltage between node 7 and ground.
Depending on the ACOUT value, VP(8,3) prints the phase of the voltage
difference between nodes 8 and 3, or the difference of the phase of
voltage at node 8 and voltage at node 3.
II(R1) prints the imaginary part of the current through R1.
.PRINT AC VM(4,2) VR(7) VP(8,3) II(R1)
Example 4
This example prints:
The magnitude of the input impedance.
The phase of the output admittance.
Several S and Z parameters.
.PRINT AC ZIN YOUT(P) S11(DB) S12(M) Z11(R)
Example 5
This example prints the DC analysis results for several different nodal
voltages and currents through:
The resistor named R1.
The voltage source named VSRC.
The drain-to-source current of the MOSFET named M1.
.PRINT DC V(2) I(VSRC) V(23,17) I1(R1) I1(M1)
Example 6
Prints the equivalent input noise.
.PRINT NOISE INOISE
Example 7
Prints the magnitude of third-order harmonic distortion, and the dB value
of the intermodulation distortion sum through the load resistor that you
specify in the .DISTO command.
.PRINT DISTO HD3 SIM2(DB)
Example 8
The command in Example 8 includes NOISE, DISTO, and AC output
variables in the same .PRINT statement.
.PRINT AC INOISE ONOISE VM(OUT) HD3
Example 9
Prints the value of pj1 with the specified function. (HSPICE
ignores .PRINT command references to nonexistent netlist part names,
and prints those names in a warning.)
.PRINT pj1=par(‘p(rd) +p(rs)‘)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
253
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PRINT
Example 10 The commands in Example 10 illustrate print statements for a derivative
function and an integrative function. The parameter can be a node
voltage or a reasonable expression.
.PRINT der=deriv('v(NodeX)')
.PRINT int=integ('v(NodeX)')
Example 11 Shows how you can use p1 and p2 as parameters in netlist. The p1 value
is 3; the p2 value is 15. You can use p1 and p2 as parameters in netlist.
.param p1=3
.print par('p1')
.print p2=par("p1*5")
Example 12 Shows the syntax for outputting the length and width of a polygon in
template format for the following models: BSIM3, BSIM4, BSIM3SOI,
BSIM4SOI, and PSP.
.print ac wpoly() lpoly()
See Also
.AC
.DC
.DCMATCH
.DISTO
.DOUT
.MEASURE (or) .MEAS
.NOISE
.PROBE
.STIM
.TRAN
Measuring the Value of MOSFET Model Card Parameters
254
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PROBE
.PROBE
Saves output variables to interface and graph data files.
Syntax
.PROBE analysis_type ov1 [ov2 ...]
.PROBE analysis_type v(inst_name.subckt_port_name)
Argument
Description
analysis_type
Type of analysis for the specified plots. Analysis types are: DC, AC, TRAN,
NOISE, or DISTO for HSPICE; ENV, HB, HBAC, HBLSP, HBNOISE,
HBTR, HBTRAN, HBXF, NOISE, or PHASENOISE for HSPICE RF.
ov1...
Output variables to plot: voltage, current, or element template (HSPICEonly variables from a DC, DCMATCH, AC, ACMATCH, TRAN, NOISE, or
DISTO analysis. .PROBE can include more than one output variable.
HSPICE RF analyses include: ENV, HB, HBAC, HBLSP, HBNOISE,
HBTR, HBTRAN, HBXF, NOISE, or PHASENOISE analysis.
inst_name
Specifies instance name.
subckt_port_name Specifies subcircuit port name.
Description
Use this command to save output variables and print to interface and graph
data files. Parameters can be node voltages, currents, elements, reasonable
expressions, and node probe instances and ports. You can include wildcards
in .PROBE commands. Inorder to save instance port nodes, you need to set
.OPTION PROBE. The .PROBE command outputs the signals to waveform files
no matter how .OPTION PROBE and .OPTION PUTMEAS are set.
Note:
For AC analysis in HSPICE, only the magnitude is saved to the
waveform file unless a complex quantity is explicitly specified.
Examples
Example 1
Saves several node voltages and an expression.
.PROBE DC V(4) V(5) V(1) beta=PAR(`I1(Q1)/I2(Q1)')
Example 2
PROBE
This syntax probes the voltage of the net connected with the Gate of
XINST1.MN0.
TRAN V2(XINST1.MN0)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
255
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PROBE
Example 3
Illustrates saving derivative and integrative functions.
* Derivative function
.PROBE der=deriv('v(NodeX)')
* Integrate function
.PROBE int=integ('v(NodeX)')
Example 4
Last section of a netlist to generate a NAND circuit, illustrating printing of
subcircuit node instances and ports. Adding .OPTION POST PROBE
limits the output to the *.lis file.
...
.subckt nand0 data clk out vdd
mna n_mid data 0 0 n w=2u l=1u
mnb out clk n_mid 0 n w=2u l=1u
mpa out clk vdd vdd p w=2u l=1u
mpb out data vdd vdd p w=2u l=1u
.ends
xa data clk out vdd nand5
v1 vdd 0 3
vdata data 0 pwl 0 0 5n 0 5.01n 3
vclk clk 0 pwl 0 0 12n 0 12.01n 3
.tran 1p 200n
.probe tran v(xa.x5x4.x4x3.clk)
.probe tran v(xa.x5x1.x4x1.clk)
.probe tran v(xa.x5x1.x4x3.data)
.opt post probe lis_new
.end
See Also
.AC
.ACMATCH
.DC
.DCMATCH
.DISTO
.DOUT
.ENV
.HB
.HBAC
.HBLSP
.HBNOISE
.HBOSC
.HBXF
.MEASURE (or) .MEAS
.NOISE
.PHASENOISE
256
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PROBE
.PRINT
.STIM
.TRAN
.OPTION PROBE
.OPTION PUTMEAS
Measuring the Value of MOSFET Model Card Parameters
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
257
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PROTECT or .PROT
.PROTECT or .PROT
Keeps models and cell libraries private as part of the encryption process in
HSPICE.
Syntax
.PROTECT
Description
Use this command to designate the start of the file section to be encrypted
when using Metaencrypt.
■
Use .UNPROTECT to end the file section that will be encrypted.
■
Any elements and models located between a .PROTECT and
an .UNPROTECT command inhibit the element and model listing from the
LIST option.
■
The .OPTION NODE nodal cross-reference and the .OP operating point
printout do not list any nodes that are contained between the .PROTECT
and .UNPROTECT commands.
Caution: If you use.prot/.unprot in a library or file that is not
encrypted you will get warnings that the file is encrypted and the
file or library is treated as a “black box.”
Note:
To perform a complete bias check and print all results in the
Outputs Biaschk Report, do not use .protect/.unprotect in
the netlist for the part that is used in .biaschk. For example: If
a model definition such as model nch is contained within
.prot/.unprot commands, in the *.lis you'll see a warning
message as follows: **warning** : model nch defined
in .biaschk cannot be found in netlist--ignored
Usage Note: The .prot/.unprot feature is meant for the encryption process
and not netlist echo suppression. Netlist and model echo suppression is on by
default since HSPICE C-2009.03. For a compact and better formatted output
(*.lis) file, use .OPTION LIS_NEW
See Also
.UNPROTECT or .UNPROT
.OPTION BRIEF
.OPTION LIS_NEW
258
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PTDNOISE
.PTDNOISE
Calculates the noise spectrum and total noise at a point in time for HSPICE RF.
Syntax
.PTDNOISE output time_value [time_delta]
+ frequency_sweep
+ [listfreq=(frequencies|none|all)] [listcount=val]
+ [listfloor=val] [listsources=on|off]
Argument
Description
output
An output node, pair of nodes, or 2-terminal elements. HSPICE RF
references the equivalent noise output to this node (or pair of nodes). Specify
a pair of nodes as V(n+,n-); only one node as V(n+, n-). If you specify only
one node, V(n+), then HSPICE RF assumes the second node is ground. You
can also specify a 2-terminal element name that refers to an existing element
in the netlist.
time_value
Time point at which time domain noise is evaluated. Specify either a time
point explicitly, such as: TIME=value, where value is either numerical or a
parameter name or a .MEASURE name associated with a time domain
.MEASURE command located in the netlist. PTDNOISE uses the time point
generated from the .MEASURE command to evaluate the noise
characteristics. This is useful if you want to evaluate noise or jitter when a
signal reaches some threshold value.
time_delta
A time value used to determine the slew rate of the time-domain
output signal. Specified as TDELTA=value. The signal slew rate is
then determined by the output signal at TIME +/- TDELTA and
dividing this difference by 2 x TDELTA. This slew rate is then used
in the calculation of the strobed jitter. If this term is omitted a
default value of 0.01 x the .SN period is assumed.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
259
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PTDNOISE
Argument
Description
frequency_sweep
Frequency sweep range for the output noise spectrum. The upper and lower
limits also specify the integral range in calculating the integrated noise value.
Specify LIN,DEC, OCT, POI, SWEEPBLOCK, DATA sweeps. Specify the
nsteps, start, and stop frequencies using the following syntax for each type
of sweep:
■
■
■
■
■
listfreq
LIN nsteps start stop
DECnsteps start stop
OCT nsteps start stopPOI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA data_name
Prints the element noise value to the .lis file. This information is only printed
if a noise spectrum is requested in a PRINT or PROBE statement. (See
PTDNOISE Output Syntax and File Format.) You can specify which
frequencies the element noise is printed. The frequencies must match the
sweep_frequency values defined in the frequency_sweep, otherwise they
are ignored.
In the element noise output, the elements that contribute the largest noise
are printed first. The frequency values can be specified with the NONE or
ALL keyword, which either prints no frequencies or every frequency defined
in frequency_sweep. Frequency values must be enclosed in parentheses.
For example:
■
listfreq=(none)
listfreq=(all)
■
listfreq=(1.0)
■
listfreq=(1.0G, 2.0G)
The default value is NONE.
■
listcount
Prints the element noise value to the .lis file, which is sorted from the largest
to smallest value. You do not need to print every noise element; instead, you
can define listcount to print the number of element noise frequencies. For
example, listcount=5 means that only the top 5 noise contributors are
printed. The default value is 1.
listfloor
Prints the element noise value to the .lis file and defines a minimum
meaningful noise value (in V/Hz1/2 units). Only those elements with noise
values larger than listfloor are printed. The default value is 1.0e-14 V/
Hz1/2.
260
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PTDNOISE
Argument
Description
listsources
Prints the element noise value to the .lis file when the element has multiple
noise sources, such as a MOSFET, which contains the thermal, shot, and 1/
f noise sources. You can specify either ON or OFF: ON prints the contribution
from each noise source and OFF does not. The default value is OFF.
Description
Periodic Time-Dependent noise analysis (PTDNOISE) calculates the noise
spectrum and the total noise at a point in time. Jitter in a digital threshold circuit
can then be determined from the total noise and the digital signal slew rate.
.MEASURE PTDNOISE allows for the measurement of these parameters:
integnoise, time-point, tdelta-value, slewrate, and strobed jitter. See Periodic
Time-Dependent Noise Analysis (.PTDNOISE) in the HSPICE User Guide: RF
Analysis for details.
Examples
The following example does a time point sweep.
.param f0 = 5.0e8
.sn tones=f0 nharms=4 trinit=10n
.PTDNOISE v(out1) TIME=lin 3 0 2n TDELTA=.1n dec 5 1e5 1e10
+ listfreq=(1e6,1e8)
+ listcount=1
+ listsources=ON
...
See Also
.HBNOISE
.SNNOISE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
261
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PZ
.PZ
Performs pole/zero analysis.
Syntax
.PZ output input
.PZ ovsrcname
Argument Description
input
Input source; the name of any independent voltage or current source.
output
Output variables, which can be:
■
■
ov
Any node voltage, V(n).
Any branch current, I(branch_name).
Output variable:
■
srcnam
a node voltage V(n), or a branch current I(element)
Input source:
■
an independent voltage or a current source name
Description
Use to perform Pole/Zero analysis. You do not need to specify .OP because the
simulator automatically invokes an operating point calculation. See Pole/Zero
Analysis in the HSPICE User Guide: Simulation and Analysis for complete
information about pole/zero analysis.
Examples
.PZ V(10) VIN
.PZ I(RL) ISORC
■
In the first pole/zero analysis, the output is the voltage for node 10 and the
input is the VIN independent voltage source.
■
In the second pole/zero analysis, the output is the branch current for the RL
branch and the input is the ISORC independent current source.
See Also
.DC
Filters Examples, for full demo netlists using the .PZ command, including:
• fbp_2.sp (bandpass LCR filter, pole/zero)
•
262
ninth.sp (active low pass filter using Laplace elements)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.PZ
•
fhp4th.sp (high-pass LCR, fourth-order Butterworth filter, pole-zero
analysis)
•
fkerwin.sp (pole/zero analysis of Kerwin’s circuit)
•
flp5th.sp (low-pass, fifth-order filter, pole-zero analysis)
•
flp9th.sp (low-pass, ninth-order FNDR, with ideal op-amps, pole-zero
analysis)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
263
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SAMPLE
.SAMPLE
Analyzes data sampling noise.
Syntax
.SAMPLE FS=freq [TOL=val] [NUMF=val]
+ [MAXFLD=val] [BETA=0|1]
Argument
Description
FS=freq
Sample frequency in hertz.
TOL
Sampling-error tolerance: the ratio of the noise power (in the highest
folding interval) to the noise power (in baseband). The default is
1.0e-3.
NUMF
Maximum number of frequencies that you can specify. The algorithm
requires about ten times this number of internally-generated
frequencies so keep this value small. The default is 100.
MAXFLD
Maximum number of folding intervals (The default is 10.0). The
highest frequency (in hertz) that you can specify is: FMAX=MAXFLD
⋅ FS
BETA
Optional noise integrator (duty cycle) at the sampling node:
■
BETA=0
no integrator
BETA=1
simple integrator (default)
If you clock the integrator (integrates during a fraction of the 1/FS
sampling interval), then set BETA to the duty cycle of the integrator.
■
Description
Use this command to acquire data from analog signals. It is used with
the .NOISE and .AC commands to analyze data sampling noise in HSPICE.
The SAMPLE analysis performs a noise-folding analysis at the output node.
See Also
.AC
.NOISE
264
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SAVE
.SAVE
Stores the operating point of a circuit in a file that you specify in HSPICE only.
Syntax
.SAVE [TYPE=type_keyword] [FILE=save_file]
+ [LEVEL=level_keyword] [TIME=save_time]
Argument
Description
TYPE=
Storage method for saving the operating point. The type can be one of
type_keyword the following. Default is NODESET.
■
■
save_file
NODESET: Stores the operating point as a NODESET command.
Later simulations initialize all node voltages to these values if you
use the .LOAD command. If circuit conditions change
incrementally, DC converges within a few iterations.
IC: Stores the operating point as an IC command. Later simulations
initialize node voltages to these values if the netlist includes
the .LOAD commands.
Name of the file that stores DC operating point data. The file name
format is save_file.ic#. Default is design.ic0.
level_keyword Circuit level at which you save the operating point. The level can be
one of the following.
■
■
■
■
save_time
ALL (default): Saves all nodes from the top to the lowest circuit
level. This option offers the greatest improvement in simulation
time.
TOP: Saves only nodes in the top-level design. Does not save
subcircuit nodes.
SELECT: Enables you to select nodes that you would like to be
reported using .PRINT or .PROBE statements.
NONE: Does not save the operating point.
Time during transient analysis when HSPICE saves the operating
point. HSPICE requires a valid transient analysis command to save a
DC operating point. The default is 0.
Description
Use this command to store the operating point of a circuit in a file that you
specify. For quick DC convergence in subsequent simulations, use the .LOAD
command to input the contents of this file. HSPICE saves the operating point by
default, even if the HSPICE input file does not contain a .SAVE command. To
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
265
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SAVE
not save the operating point, specify .SAVELEVEL=NONE. You can save the
operating point data as either an .IC or a .NODESET command. A parameter
or temperature sweep saves only the first operating point.
The .SAVE command only saves one bias point to a file.
Note:
To save multiple node voltages at different timesteps, it is
preferable to use the .OP command.
MP and DP do not support saving and loading *.ic files. If a netlist contains
.save or .load commands, then -mp and -dp are disabled.
Examples
Example 1
This example saves the operating point corresponding to .TEMP -25 to a
file named my_design.ic0.
.TEMP -25 0 25
.SAVE TYPE=NODESET FILE=my_design.ic0 LEVEL=ALL
+ TIME=0
Example 2
In this example statement, only the four specified signals are printed in
the test.ic0 file.
.SAVE LEVEL=SELECT FILE='test.ic0'
.probe v(in) v(x1.clk) v(x1.xpll.4gout) v(out_n)
Example 3
This example appears in a file where there are eight end's where there
are .SAVE lines in every other .end (four total). The save_file flag is
’6230_lrmf.ic’. The resultant files are:
6230_lrmf.ic0
6230_lrmf.ic1
6230_lrmf.ic2
6230_lrmf.ic3
.SAVE TYPE=IC TIME=1.72323e-09 FILE='6230_lmrf.ic'
See Also
.IC
.LOAD
.NODESET
.OP
.PRINT
.PROBE
266
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SENS
.SENS
Determines DC small-signal sensitivities of output variables for circuit
parameters.
Syntax
.SENS ov1 [ov2 ...]
Argument
Description
ov1 ov2 ...
Branch currents or nodal voltage for DC component-sensitivity
analysis
Description
Use this command to determine DC small-signal sensitivities of output
variables for circuit parameters.
If the input file includes a .SENS command, HSPICE determines DC smallsignal sensitivities for each specified output variable relative to every circuit
parameter. The sensitivity measurement is the partial derivative of each output
variable for a specified circuit element measured at the operating point and
normalized to the total change in output magnitude. Therefore, the sum of the
sensitivities of all elements is 100%. DC small-signal sensitivities are
calculated for:
■
resistors
■
voltage sources
■
current sources
■
diodes
■
BJTs (including Level 4, the VBIC95 model)
■
MOSFETs (Level49 and Level53, Version=3.22).
Note:
The only BSIM3 model version supported in sensitivity analysis
is the BSIM3V3.22 model. BSIMV3.2, BSIM3V3.24, and
BSIM3V3.3 models are not supported.
You can perform only one .SENS analysis per simulation. Only the last .SENS
command is used in case more than one is present. The others are discarded
with warnings. The amount of output generated from a .SENS analysis is
dependent on the size of the circuit.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
267
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SENS
Examples
In Example 1, the .SENS v(2) command is used to find out how sensitive the
voltage at node 2 is to change at any element value.
For sensitivity analysis only one element is changed at a time while all other
element values are retained at their original value. The output of the .SENS
v(2) command appears in the list file as follows:
Example 1
v1 1 0 1
r1 1 2 1k
r2 2 0 1k
.SENS v(2)
.end
In Example 2, the element sensitivity column lists the absolute change in V(2)
when the element value is changed by unity. As shown, an element sensitivity
of -250.0000u for element r1 indicates that v(2) decreases by 250uv when R1
is increased from 1000 ohms to 1001 ohms. Similarly, an element sensitivity of
500.0000m for element v1 indicates that v(2)increases by 500mv when v1
increases by 1V.
The normalized sensitivity column lists the absolute change in v(2) when the
element value is increased by 1%. As shown for element r1, the normalized
sensitivity of -2.5000m indicates that v(2) decreases by 2.5mv when the value
of r1 is increased by 1%.
Example 2
dc sensitivities of output v(2)
element element element normalized
name value sensitivity sensitivity
(volts/unit) (volts/percent)
0:r1 1.0000k -250.0000u -2.5000m
0:r2 1.0000k 250.0000u 2.5000m
0:v1 1.0000 500.0000m 5.0000m
Note:
In both columns, a negative sign indicates a decrease and a
positive sign indicates an increase in the output variable (in this
case, v(2)).
See Also
.DC
268
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE
.SHAPE
Defines a shape to be used by the HSPICE field solver.
Syntax
.SHAPE snameShape_Descriptor
Argument
Description
sname
Shape name.
Shape_Descriptor One of the following:
■
■
■
■
■
Rectangle
Circle
Strip
Polygon
Trapezoid
Description
Use this command to define a shape. The field solver uses the shape to
describe a cross-section of the conductor.
See Also
.SHAPE (Defining Rectangles)
.SHAPE (Defining Circles)
.SHAPE (Defining Polygons)
.SHAPE (Defining Strip Polygons)
.SHAPE (Defining Trapezoids)
.FSOPTIONS
.LAYERSTACK
.MATERIAL
Transmission (W-element) Line Examples
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
269
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE (Defining Rectangles)
.SHAPE (Defining Rectangles)
Defines a rectangle to be used by the HSPICE field solver.
Syntax
.SHAPE RECTANGLE WIDTH=val HEIGHT=val [NW=val] [NH=val]
Argument
Description
WIDTH
Width of the rectangle (size in the x-direction).
HEIGHT
Height of the rectangle (size in the y-direction).
NW
Number of horizontal (x) segments in a rectangle with a specified width.
NH
Number of vertical (y) segments in a rectangle with a specified height.
Description
Use this keyword to define a rectangle. Normally, you do not need to specify the
NW and NH values because the field solver automatically sets these values,
depending on the accuracy mode. You can specify both values or only one of
these values and let the solver determine the other.
y
Width
Height
Origin
(0,0)
Figure 9
270
x
Coordinates of a Rectangle
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE (Defining Circles)
.SHAPE (Defining Circles)
Defines a circle to be used by the HSPICE field solver.
Syntax
.SHAPE CIRCLE RADIUS=val [N=val]
Argument
Description
RADIUS
Radius of the circle.
N
Number of segments to approximate a circle with a specified radius.
Description
Use this keyword to define a circle in the field solver. The field solver
approximates a circle as an inscribed regular polygon with N edges. The more
edges, the more accurate the circle approximation is.
Do not use the CIRCLE descriptor to model actual polygons; instead use the
POLYGON descriptor.
Normally, you do not need to specify the N value because the field solver
automatically sets this value, depending on the accuracy mode. But you can
specify this value if you need to
y
Origin
Radius
Starting vertex
of the inscribed
polygon
(0,0)
Figure 10
x
Coordinates of a Circle
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
271
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE (Defining Polygons)
.SHAPE (Defining Polygons)
Defines a polygon to be used by the HSPICE field solver.
Syntax
.SHAPE POLYGON VERTEX=(x1y1x2y2 ...)
+ [N=(n1,n2,...)]
Argument
Description
VERTEX
(x, y) coordinates of vertices. Listed either in clockwise or counterclockwise direction.
N
Number of segments that define the polygon with the specified x and y
coordinates. You can specify a different N value for each edge. If you
specify only one N value, then the field solver uses this value for all
edges.For example, the first value of N, n1, corresponds to the number of
segments for the edge from (x1 y1) to (x2 y2).
Description
Use this command to define a polygon in a field solver. The specified
coordinates are within the local coordinate with respect to the origin of a
conductor.
y
Origin
(0,0)
Figure 11
x
Coordinates of a Polygon
Examples
Example 1 demonstrates a rectangular polygon using the default number of
segments.
Example 1
.SHAPE POLYGON VERTEX=(1 10 1 11 5 11 5 10)
272
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE (Defining Polygons)
The rectangular polygon specified in Example 2 uses five segments for each
edge.
Example 2
.SHAPE POLYGON VERTEX=(1 10 1 11 5 11 5 10)
+ N=5
Example 3 shows how rectangular polygon uses different number of segments
for each edge.
Example 3
.SHAPE POLYGON VERTEX=(1 10 1 11 5 11 5 10)
+ N=(5 3 5 3)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
273
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE (Defining Strip Polygons)
.SHAPE (Defining Strip Polygons)
Defines a strip polygon to be used by the HSPICE field solver.
Syntax
.SHAPE STRIP WIDTH=val [N=val]
Argument
Description
WIDTH
Width of the strip (size in the x-direction).
N
Number of segments that define the strip shape with the specified
width.
Description
Use this command to define a strip polygon in a field solver. Normally, you do
not need to specify the N value because the field solver automatically sets this
value, depending on the accuracy mode. But you can specify this value if you
need to.
The field solver (filament method) does not support this shape.
y
Width
Origin
(0,0)
Figure 12
274
x
Coordinates of a Strip Polygon
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SHAPE (Defining Trapezoids)
.SHAPE (Defining Trapezoids)
Defines a trapezoid to be used by the HSPICE field solver.
Syntax
.SHAPE TRAPEZOID TOP=val BOTTOM=val HEIGHT=val
+ [NW=val] [NH=val]
Argument
Description
TOP
Top edge length of the trapezoid (size in the x-direction).
BOTTOM
Bottom edge length of the trapezoid (size in the x-direction).
HEIGHT
Height of the trapezoid (size in the y-direction).
NW
Number of horizontal (x) segments in a trapezoid with a specified top and
bottom.
NH
Number of vertical (y) segments in a trapezoid with a specified height.
Description
Use this keyword to define a trapezoid. Normally, you do not need to specify the
NW and NH values because the field solver automatically sets these values,
depending on the accuracy mode. You can specify both values or only one of
these values to let the solver determine the other.
Figure 13
Coordinates of a Trapezoid
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
275
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SN
.SN
In HSPICE RF, Shooting Newton provides two syntaxes. Syntax #1 is
recommended when you are using/making Time Domain sources and
measurements (for example, going from .TRAN to .SN). Syntax #2 effectively
supports Frequency Domain sources and measurements (and should be used,
for example, when going from .HB to .SN).
Syntax
Syntax #1
.SN TRES=Tr PERIOD=T [TRINIT=Ti] [SWEEP parameter_sweep]
+ [MAXTRINITCYCLES=integer] [NUMPEROUT=val]
Syntax #2
.SN TONE=F1 NHARMS=N [TRINIT=Ti] [SWEEP parameter_sweep]
+ [MAXTRINITCYCLES=integer] [NUMPEROUT=val]
Argument
Description
TRES
Time resolution to be computed for the steady-state waveforms (in
seconds).
PERIOD
Expected period T (seconds) of the steady-state waveforms. Enter an
approximate value when using for oscillator analysis. The period of the
steady-state waveform may be entered either as PERIOD or its
reciprocal, TONE.
TRINIT
Transient initialization time. If not specified, the transient initialization
time will be equal to the period (for Syntax 1) or the reciprocal of the tone
(for Syntax 2).
SWEEP
Parameter sweep. As in all main analyses in HSPICE RF such
as .TRAN, .HB, etc., you can specify LIN, DEC, OCT, POI,
SWEEPBLOCK, DATA, MONTE, or OPTIMIZE.
MAXTRINITCYCLES
SN stabilization simulation and frequency detection is stopped when the
simulator detects that maxtrinitcycles have been reached in the
oscnode signal, or when time=trinit, whichever comes first. Minimum
cycles is 1.
TONE
Fundamental frequency (in Hz).
276
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SN
Argument
Description
NHARMS
Specifies the number of high-frequency harmonic components to
include in the analysis. NHARMS defaults to PERIOD/TRES rounded to
nearest integer. NHARMS is required to run subsequent SNAC,
SNNOISE, SNXF, and PHASENOISE analyses. When using Syntax #1,
NHARMS is computed automatically as NHARMS=Round(PERIOD/
TRES).
NUMPEROUT
Allows you to dump more than one period of output to ease waveform
viewing. (Your eye doesn’t have to struggle in the viewer to connect the
end of a waveform period to its beginning.) By default, SN analysis only
dumps one period of output.
Description
Shooting-Newton adds analysis capabilities for PLL components, digital
circuits/logic, such as ring oscillators, frequency dividers, phase/frequency
detectors (PFDs), and for other digital logic circuits and RF components that
require steady-state analysis, but operate with waveforms that are more square
wave than sinusoidal. Refer to the HSPICE User Guide: RF Analysis, SteadyState Shooting Newton Analysis.
In addition to all .TRAN options, .SN analysis supports the following options:
■
.OPTION LOADSNINIT
■
.OPTION SAVESNINIT
■
.OPTION SNACCURACY
■
.OPTION SNMAXITER
See Also
.SNAC
.SNFT
.SNNOISE
.SNOSC
.SNXF
.OPTION LOADSNINIT
.OPTION SAVESNINIT
.OPTION SNACCURACY
.OPTION SNMAXITER (or) SN_MAXITER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
277
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNAC
.SNAC
Runs a frequency sweep across a range for the input signal based on a
Shooting Newton algorithm.
Syntax
.SNAC frequency_sweep
Argument
Description
frequency_sweep
Frequency sweep range for the input signal (also referred to as the
input frequency band (IFB) or fin). You can specify LIN, DEC, OCT,
POI, or SWEEPBLOCK. Specify the nsteps, start, and stop times
using the following syntax for each type of sweep:
■
■
■
■
■
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
Description
The frequency_sweep runs across a range for the input signal based on a
Shooting Newton algorithm. For more information, see Shooting Newton AC
Analysis (.SNAC) in the HSPICE User Guide: RF Analysis.
Examples
VSRC node1 node2 0 SNAC 1 45
.SNAC DEC 10 1k 10K
See Also
.HBAC
.SN
.SNNOISE
278
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNFT
.SNFT
Calculates the Discrete Fourier Transform (DFT) value used for Shooting
Newton analysis. Numerical parameters (excluding string parameters) can be
passed to the .SNFT command.
Syntax
Syntax # 1 Alphanumeric input
.SNFT output_var [START=value] [STOP=value]
+ [NP=value] [FORMAT=keyword]
+ [WINDOW=keyword] [ALFA=value]
+ [FREQ=value] [FMIN=value] [FMAX=value]
Syntax #2 Numerics and expressions
.SNFT output_var [START=param_expr1] [STOP=param_expr2]
+ [NP=param_expr3] [FORMAT=keyword]
+ [WINDOW=keyword] [ALFA=param_expr4]
+ [FREQ=param_expr5] [FMIN=param_expr6] [FMAX=param_expr7]
Argument
Description
output_var
Any valid output variable, such as voltage, current, or power.
START
Start of the output variable waveform to analyze. Defaults to the START value in
the .SN command, which defaults to 0.
FROM
Alias for START in .SNFT commands.
STOP
End of the output variable waveform to analyze. Defaults to the TSTOP value in
the .SN command.
TO
Alias for STOP, in .SNFT commands.
NP
Number of points to use in the SNFT analysis. NP must be a power of 2. If NP is
not a power of 2, HSPICE automatically adjusts it to the closest higher number that
is a power of 2. The default is 1024.
FORMAT
Output format:
■
■
NORM= normalized magnitude (default)
UNORM=unnormalized magnitude
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
279
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNFT
Argument
Description
WINDOW
Window type to use:
■
■
■
■
■
■
■
■
RECT=simple rectangular truncation window (default).
BART=Bartlett (triangular) window.
HANN=Hanning window.
HAMM=Hamming window.
BLACK=Blackman window.
HARRIS=Blackman-Harris window.
GAUSS=Gaussian window.
KAISER=Kaiser-Bessel window.
ALFA
Parameter to use in GAUSS and KAISER windows to control the highest side-lobe
level, bandwidth, and so on. 1.0 <= ALFA <= 20.0The default is 3.0
FREQ
Frequency to analyze. If FREQ is non-zero, the output lists only the harmonics of
this frequency, based on FMIN and FMAX. HSPICE also prints the THD for these
harmonics. The default is 0.0 (Hz).
FMIN
Minimum frequency for which HSPICE prints SNFT output into the listing file. THD
calculations also use this frequency. T=(STOP-START) The default is 1.0/T (Hz).
FMAX
Maximum frequency for which HSPICE prints SNFT output into the listing file. THD
calculations also use this frequency. The default is 0.5*NP*FM IN (Hz).
Description
Use this command to calculate the Discrete Fourier Transform (DFT) spectrum
analysis values for Shooting Newton analysis. It uses internal time point values
to calculate these values. A DFT uses sequences of time values to determine
the frequency content of analog signals in circuit simulation. You can pass
numerical parameters/expressions (but no string parameters) to the .SNFT
command. The output goes to a file with extension .snft#.
You can specify only one output variable in an .SNFT command. The following
is an incorrect use of the command because it contains two variables in
one .SNFT command:
280
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNFT
Examples
Example 1
Correctly designates the variables per .SNFT command.
.SNFT v(1)
.SNFT v(1,2) np=1024 start=0.3m stop=0.5m freq=5.0k
+ window=kaiser alfa=2.5
.SNFT I(rload) start=0m to=2.0m fmin=100k fmax=120k
+ format=unorm
.SNFT par(‘v(1) + v(2)’) from=0.2u stop=1.2u
+ window=harris
Example 2
Generates a .snft0 file for the SNFT of v(1) and a .snft1 file for the SNFT
of v(2).
.SNFT v(1) np=1024
.SNFT v(2) np=1024
See Also
.SN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
281
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNNOISE
.SNNOISE
Runs a periodic, time-varying AC noise analysis based on a Shooting Newton
algorithm.
Syntax
.SNNOISE [output] [insrc] [frequency_sweep]
+ [n1, +/-1]
+[listfreq=(frequencies|none|all)> [listcount=val]
+[listfloor=val] [listsources=on|off]
Argument
Description
output
Output node, pair of nodes, or 2-terminal element that the equivalent
noise output references.
insrc
Input source.
frequency_sweep Frequency sweep range for the input signal. You can specify LIN, DEC,
OCT, POI, SWEEPBLOCK, DATA, MONTE, or OPTIMIZE sweeps.
n1, +/-
Index term defining the output frequency band at which the noise is
evaluated. The output frequency is computed according to fout=|n1*f1 +/
- fin|, where f1 is the fundamental tone (inverse of fundamental period)
and fin is from the frequency sweep.
listfreq
Prints the element noise value to the .lis file; the default is none.
listcount
Prints the element noise value to the .lis file, sorted from the largest to
smallest value.
listfloor
Prints the element noise value to the .lis file and defines a minimum
meaningful noise value. Only those elements with noise values larger
than listfloor are printed. The default value is 1.0e-14 V/sqrt(Hz).
listsources
Prints the element noise value to the .lis file when the element has
multiple noise sources. The default is off.
Description
The functionality for the .SNNOISE command to is similar to the Harmonic
Balance (HBNOISE command) for periodic, time-varying AC noise analysis, but
282
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNNOISE
the Shooting Newton-based algorithm completes the analysis in a much faster
run time with the same result.
Examples
.SNNOISE V(n1,n2) RIN DEC 10 1k 10k 0 -1
See Also
.HBNOISE
.SN
.SNAC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
283
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNOSC
.SNOSC
Performs oscillator analysis on autonomous (oscillator) circuits. As with regular
Shooting Newton analysis, input might be specified in terms of time or
frequency values.
Syntax
Syntax #1
.SNOSC TONE=F1 NHARMS=H1 [TRINIT=Ti] OSCNODE=N1
+[MAXTRINITCYCLES=N][SWEEP PARAMETER_SWEEP]
Syntax #2
.SNOSC TRES=Tr PERIOD=Tp [TRINIT=Tr] OSCNODE=N1
+[MAXTRINITCYCLES=I] SWEEP PARAMETER_SWEEP
284
Argument
Description
TONE
Approximate value for oscillation frequency (Hz). The search
for an exact oscillation frequency begins from this value.
NHARMS
Number of harmonics to be used for oscillator SN analysis.
OSCNODE
Node used to probe for oscillation conditions. This node is
automatically analyzed to search for periodic behavior near
the TONE or PERIOD value specified.
TRINIT
Transient initialization time. If not specified, the transient
initialization time is equal to the period (for Syntax 1) or the
reciprocal of the tone (for Syntax 2). For oscillators we
recommend specifying a transient initialization time since the
default initialization time is usually too short to effectively
stabilize the circuit.
MAXTRINITCYCLES
SN stabilization simulation and frequency detection is
stopped when the simulator detects that
MAXTRINITCYCLES have been reached in the oscnode
signal, or when time=trinit, whichever comes first.
Minimum cycles is 1.
TRES
Time resolution to be computed for the steady-state
waveforms (in seconds). The period of the steady-state
waveform may be entered either as PERIOD or its reciprocal,
TONE.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNOSC
Argument
Description
PERIOD
Expected period T (seconds) of the steady-state waveforms.
Enter an approximate value when using for oscillator analysis.
SWEEP
Type of sweep. You can sweep up to three variables. You can
specify either LIN, DEC, OCT, POI, SWEEPBLOCK, DATA,
OPTIMIZE, or MONTE. Specify the nsteps, start, and stop
frequencies using the following syntax for each type of sweep:
■
■
■
■
■
■
■
■
LIN nsteps start stop
DEC nsteps start stop
OCT nsteps start stop
POI nsteps freq_values
SWEEPBLOCK nsteps freq1 freq2 ... freqn
DATA=dataname
OPTIMIZE=OPTxxx
MONTE=val
Description
Use this command to invoke oscillator analysis on autonomous (oscillator)
circuits. The SNOSC command is very effective for ring oscillator circuits, and
oscillators that operate with piecewise linear waveforms (HBOSC is superior for
sinusoidal waveforms). As with the Harmonic Balance approach, the goal is to
solve for the additional unknown oscillation frequency. This is accomplished in
Shooting Newton by considering the period of the waveform as an additional
unknown, and solving the boundary conditions at the waveform endpoints that
coincide with steady-state operation. As with regular Shooting Newton
analysis, input might be specified in terms of time or frequency values. See the
examples, below.
Examples
Example 1
Performs an oscillator analysis searching for periodic behavior after an
initial transient analysis of 10 ns. This example uses nine harmonics
while searching for a oscillation at the gate node.
.SNOSC tone=900Meg nharms=9 trinit=10n oscnode=gate
Example 2
Performs an oscillator analysis searching for frequencies in the vicinity of
2.4 Ghz. This example uses 11 harmonics and a search at the drainP.
.SNOSC tone=2400MEG nharms=11 trinit=20n oscnode=drainP
Example 3
Presents another equivalent method to define the OSCNODE
information through a zero-current source. Example 3 is identical to
Example 2, except that the OSCNODE information is defined by a current
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
285
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNOSC
source in the circuit. Only one such current source is needed and its
current source must be 0.0 with the SNOSC OSCNODE identified by the
SNOSCVPROBE keyword.
ISRC drainP 0 SNOSCVPROBE
.SNOSC tone = 2.4 G nharms = 1 trinit=20n
See Also
.HB
.OPTION HBFREQABSTOL
.OPTION HBFREQRELTOL
.OPTION HBOSCMAXITER (or) HBOSC_MAXITER
.OPTION HBPROBETOL
.OPTION HBTRANFREQSEARCH
.OPTION HBTRANINIT
.OPTION HBTRANPTS
.OPTION HBTRANSTEP
.PRINT
.PROBE
286
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNXF
.SNXF
Calculates the transfer function from the given source in the circuit to the
designated output.
Syntax
.SNXF out_varfreq_sweep
Argument
Description
out_var
I(2_port_elem) or V(n1<,n2>)
freq_sweep
Sweep of type LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the
nsteps, start, and stop times using the following syntax for each
type of sweep:
■
LIN nsteps start stop
DEC nsteps start stop
■
OCT nsteps start stop
■
POI nsteps freq_values
■
SWEEPBLOCK = BlockName
Specify the frequency sweep range for the output signal. HSPICE
RF determines the offset frequency in the input sidebands; for
example,f1 = abs(fout - k*f0) s.t. f1<=f0/2The f0 is the steady-state
fundamental tone and f1 is the input frequency.
■
Description
Use this command in HSPICE RF to calculate the transfer function from the
given source in the circuit to the designated output. The functionality for the
.SNXF command is similar to the Harmonic Balance (.HBXF) command
for periodic, time-varying AC noise analysis, but the Shooting Newton based
algorithm completes the analysis in a much faster run time with the same
result.
Examples
In this example, the trans-impedance from isrc to v(1)is calculated based on
the HB analysis.
.hb tones=1e9 nharms=4
.snxf v(1) lin 10 1e8 1.2e8
.print snxf tfv(isrc) tfi(n3)
See Also
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
287
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SNXF
.HBAC
.HBNOISE
.HBOSC
.PRINT
.PROBE
288
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STATEYE
.STATEYE
Enables use of statistical eye diagram analysis.
Syntax
.STATEYE T=time_interval Trf=rise_fall_time
+ [Tr=rise_time] [Tf=fall_time]
+ Incident_port=idx1, [idx2, ... idxN]
+ Probe_port=idx1, [idx2, ... idxN]
+ [Tran_init=n_periods]
+ [V_low=val] [V_high=val]
+ [T_resolution=n] [V_resolution=n]
+ [TD_In=val] [TD_Probe=val]
+ [VD_range=val] [TD_NUI=n] [Edge=1|2]
+ [Pattern_max=n] [Pattern_repeat=n]
+ [SAVE_TR=ascii] [LOAD_TR=ascii] [SAVE_DIR=string]
+ [Ingore_Bits=n] [AMIGW_Nbit=n]
Argument
Description
T
Time (in seconds) of single bit width of the incident signal, normally
referred as Unit Interval (UI)
Trf
Single value (in seconds) to set both the rise and fall times of the incident
pulse
Tr
Rise time (in seconds) of the incident port
Tf
Fall time (in seconds) of the incident port
Incident_port
An array of the index numbers of the incident port elements
Probe_port
An array of the index numbers of the probing port elements
V_low
Low voltage level of the incident pulse. The value is used when the
voltage level is not specified in the incident port(s).
V_high
High voltage level of the incident pulse. The value is used when the
voltage level is not specified in the incident port(s).
Tran_init
An integer number that specifies the numbers of unit intervals (T) that is
used by the initial transient analysis to determine the response of the
system. Default value is 60.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
289
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STATEYE
Argument
Description
T_resolution
An integer number used to specify the probability density function (PDF)
image resolution of the time axis. Default value is 200.
TD_In
Applies specified time delay to the incident pulse/step in the initial
transient analysis. Default value is 0 (no delay).
TD_Probe
When a positive time value is specified, StatEye only uses initial transient
analysis waveforms after the specified time for the eye diagram
generation. Default value is 0.
V_resolution
An integer number used to specify the probability density function (PDF)
image resolution of the voltage axis. Default value is 200.
VD_range
Specifies voltage display (output data) range. By default, the .StatEye
analysis engine automatically determines the optimum voltage display
range. Specifying VD_range can enlarge the display range.
TD_NUI
An integer number to specify time display range relative to the unit
interval. Default value is 2 to display a single eye. TD_NUI value may be
from 1 to 5. The higher value requires a larger data size.
EDGE
Number of edges to be used.
■
■
1: Conventional statistical eye generation using the single pulse
response (default).
2: Double-edge mode. The rising and falling edges are evaluated
separately.
PATTERN_MAX
Limits the number of bits to be examined for a custom bit pattern specified
with LFSR/PAT in incident Port-element(s). For example, if
PATTERN_MAX=100 is specified, StatEye examines only the first 100 bits
in the LFSR/PAT sources. This keyword is especially effective when
LFSR is used with very high (over 20-bit) feedback tap(s) since it
generates an extremely long bit stream. The default value of the
PATTERN_MAX is 221 to provide sufficient accuracy for most cases. When
PATTERN_MAX is not specified or PATTERN_MAX=0 is specified, StatEye
examines all the given pattern(s).
PATTERN_REPEAT
When a positive number, n, is specified, .StatEye repeats pattern
examination n times until the number of bits hits the Pattern_max value.
Default=0 (no repeats).
SAVE_TR=ascii
Saves initial transient data in text files.
290
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STATEYE
Argument
Description
LOAD_TR=ascii
Loads initial transient data from text files when available.
SAVE_DIR=string
Specifies a target directory other than the one specified by the -o
command option for the SAVE_TR and LOAD_TR transient files.
Ignore_Bits=n
When a positive number is specified, StatEye's pattern-specific eye
diagram generation process ignores the first n bits. The value is
overridden by one specified in the AMI parameter file when one exists for
each probe port.
AMIGW_Nbit=n
Specifies the number of bits per each AMI_GetWave call (see amicheck
Output). For example, when a given pattern has 10,000 bits and
AMIGW_Nbit=1000, StatEye sequentially calls AMI_GetWave 10 times
with stream waveform of 1000 bits.
The default value is 1000. For more details about AMI_GetWave, see
chapter 10 of the IBIS version 5.0 specification.
Description
Use this command to perform statistical eye analysis to evaluate high-speed
serial interfaces.
Note:
The .STATEYE command is invoked using the hspicerf
executable on the command line for this release, not hspice.
However, running a statistical eye analysis only requires an
HSPICE license token.
The statistical eye diagram is a fundamental performance metric for high-speed
serial interfaces in the bit error rate (BER). When setting up a Statistical Eye
Analysis, the Port element is used to designate the incident (input) and probe
(output) ports for the system to be analyzed. Ports can be specified as singleended or mixed mode. Random jitter can be applied to each incident and probe
point in the system.Each incident port acts as random bit pattern source with
specified voltage magnitude. If an incident port element does not have a time
domain voltage magnitude specification, the default values, V_high=1.0,
V_low=-1.0 are used.Probe ports are used as observation points where
.PRINT, .PROBE, and .MEASURE commands can be defined.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
291
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STATEYE
Examples
.STATEYE T=400p Trf=20p
+ incident_port= 1, 2
+ probe_port= 3, 4
+ Rj = 5p, 5p, 2p, 2p tran_init= 50
+ T_resolution= 300 V_resolution= 300
See Also
.MEASURE (or) .MEAS
.PRINT
.PROBE
Statistical Eye Analysis
292
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STIM
.STIM
Uses the results (output) of one simulation as input stimuli in a new simulation
in HSPICE.
Syntax
General Syntax:
.STIM [tran|ac|dc] PWL|DATA|VEC
+ [filename=output_filename ...]
PWL Source Syntax (Transient Analysis Only)
.STIM
[tran] PWL [filename=output_filename]
+
[name1=] ovar1 [node1=n+] [node2=n-]
+
[[name2=]ovar2 [node1=n+] [node2=n-] ...]
+
[from=val] [to=val] [npoints=val]
.STIM
[tran] PWL [filename=output_filename]
+
[name1=] ovar1 [node1=n+] [node2=n-]
+
[[name2=]ovar2 [node1=n+] [node2=n-] ...]
+
indepvar=[(]t1 [t2 ...[)]]
Data Card Syntax
.STIM
[tran|ac|dc] DATA [filename=output_filename]
+
dataname [name1=] ovar1
+
[[name2=]ovar2 ...] [from=val] [to=val]
+
[npoints=val] [indepout=val]
.STIM
[tran | ac | dc] DATA [filename=output_filename]
+
dataname [name1=] ovar1
+
[[name2=]ovar2 ...] indepvar=[(]t1 [t2 ...[)]]
+
[indepout=val]
Digital Vector File Syntax (Transient Analysis Only)
.STIM [tran] VEC [filename=output_filename]
+
vth=val vtl=val [voh=val] [vol=val]
+ [name1=] ovar1 [[name2=] ovar2 ...]
+ [from=val] [to=val] [npoints=val]
.STIM [tran] VEC [filename=output_filename]
+
vth=val vtl=val [voh=val] [vol=val]
+ [name1=] ovar1 [[name2=] ovar2 ...]
+ indepvar=[(]t1 [t2 ...[)]]
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
293
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STIM
Argument
Description
tran | ac | dc Simulation type: transient, AC, or DC.
filename
Output file name. If you do not specify a file, HSPICE uses the input filename.
name1
PWL Source Name that you specify. The name must start with V (for a voltage
source) or I (for a current source). Or—Name of a parameter of the data card to
generate.
ovar1
Output variable that you specify. ovar can be:
■
Node voltage.
Element current.
■
Parameter string. If using a parameter string you must specify name1.
For example: v(1), i(r1), v(2,1), par(’v(1)+v(2)’)
■
dataname
Name of the data card to generate.
node1
Positive terminal node name.
node2
Negative terminal node name.
from
Time to start output of simulation results. For transient analysis, it uses the time
units that you specified. Cannot use with indepvar.
npoints
Number of output time points or independent-variable points.
to
Time to terminate output of simulation results. For transient analysis, it uses the
time units that you specified. The from value can be greater than the to value.
Cannot use with indepvar.
indepvar
Dispersed (independent-variable) time points. Specify dispersed time points in
increasing order. Replaces the “from” and “to” construct.
indepout
Indicates whether to generate the independent variable column.
■
indepout, indepout=1, or on, produces the independent variable column. You
can specify the independent-variables in any order.
■
indepout= 0 or off (default) does not create an independent variable column.
You can place the indepout field anywhere after the ovar1 field.
vth
High voltage threshold.
vtl
Low voltage threshold.
294
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STIM
Argument
Description
voh
Logic-high voltage for each output signal.
vol
Logic-low voltage for each output signal.
Description
Use this command to reuse the results (output) of one simulation as input
stimuli in a new simulation.
The .STIM command specifies:
■
Expected stimulus (PWL Source, DATA CARD, or VEC FILE).
■
Signals to transform.
■
Independent variables.
One .STIM command produces one corresponding output file.
For additional information, see “Reusing Simulation Output as Input Stimuli” in
the HSPICE User Guide: Simulation and Analysis.
Examples
In Example 1, the .STIM command creates a file “test.pwl0_tr0”, having a
voltage source “v0” applied between nodes neg and 0 (ground). It has a PWL
source function based on the voltage of node n0 during the time 0.0ns to 5.0ns
with 10 points.
Example 1
.stim tran pwl filename=test v0=v(n0) node1=neg
+ node2=0 from=0.0ns to=5ns npoints=10
Example 2: In this example the “from and to” construct is used:
.stim tran data filename=new PWL v(2) from=start to=end
Example 3: In this example, the indepvar construct replaces “from and to”;
using both constructs results in an error.
.stim tran pwl filename=new v(2) indepvar=(2n 3n 4n)
See Also
.DOUT
.MEASURE (or) .MEAS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
295
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STIM
.PRINT
.PROBE
296
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STORE
.STORE
Starts a store operation to create checkpoint files describing a running process
during transient analysis (HSPICE).
Syntax
.STORE [file=checkpoint_file] [time=time1]
+ [repeat=checkpoint_interval]
Argument
Description
file=checkpoint_file Checkpoint files are saved as checkpoint_file.store.gz and
checkpoint_file.tar; if not specified, the default checkpoint file name prefix
is same as the HSPICE output file.
time=time1
Collects checkpoint data beginning at time1 after the start of transient
analysis. It then updates the checkpoint data every 21,600 wall-clock
seconds if no checkpoint interval is specified.
repeat=
If you specify a nonzero checkpoint_interval, new checkpoint data is
checkpoint_interval collected at every checkpoint_interval, starting at transient time=0 and
overwriting previous interval checkpoint data. If a nonzero time1 is
specified, checkpoint data is collected at time1 + checkpoint_interval * n,
where n is an integer. Checkpoint_interval is always calculated based on
time1. If repeat=0, the store operation is disabled. If you set both time=0
and repeat=0, checkpoint data is saved at transient time=0 only.
trantime=flag
■
If flag is not equal to 1 (! =1), or trantime is not specified, time1 and
checkpoint_interval are taken as wall-clock time.
■
If flag=1, time1 and checkpoint_interval will be taken as simulation time;
checkpoint will start at simulation time time1+checkpoint_interval*n.
To avoid too-frequent checkpoints, checkpoint_interval adjusts
automatically if the wall-clock time interval of the store operation is less
than 7200 seconds.
Description
Use this command in a netlist to trigger a restore operation by creating
checkpoint files describing a running process during transient analysis; the
operating system can later reconstruct the process from the contents of this
file. This feature is not supported in HSPICE-RF.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
297
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STORE
The shortest period for a checkpoint_interval is 7,200 seconds, anything
shorter than that defaults to 7,200 seconds automatically.
If the netlist contains more than one .store statement, only the last statement
takes effect.
The restore operation is done on the command-line with the restore keyword.
See Chapter 1, HSPICE and HSPICE RF Application Commands for more
information. For usage requirements and additional information, see Storing
and Restoring Checkpoint Files (HSPICE) in the HSPICE User Guide:
Simulation and Analysis.
Examples
Example 1: Checkpoint data is saved at 50 wall-clock seconds of transient
analysis in chk_50.store.gz and chk_50.tar files. Checkpoint data is
also updated every 21,600 wall-clock seconds.
.store file=chk_50 time=50
Example 2: After transient analysis starts, the store operation occurs at 7,200
wall-clock seconds, 14,400 wall-clock seconds, 21,600 wall-clock seconds, and
so on. Each new time interval overwrites previous interval checkpoint files.
.store repeat=7200
Example 3: After transient analysis starts, the store operation occurs at 300
wall-clock seconds, 7,500 wall-clock seconds, 14,700 wall-clock seconds, and
so on. Each new time interval overwrites previous interval check-point files.
.store time=300 repeat=7200
Example 4: This statement turns off the store operation.
.store repeat=0
Example 5: The store operation saves the data at the time transient analysis
begins in outputfile.store.gz and outputfile.tar files.
.store time=0 repeat=0
Example 6: The first store operation starts at simulation time 1ns, then repeats
every 10ns. The repeat value is adjusted if the wall-clock time interval of the
store operation less than 7,200 seconds.
store trantime=1 time=1n repeat=10n
298
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.STORE
Example 7: The first store operation starts at simulation time 10ns, then repeat
every 10ns. The repeat value is adjusted if the wall-clock time interval of the
store operation is less than 7,200 seconds.
.store trantime=1 repeat=10n
Example 8: The store operation starts at simulation time 0.00001s, but does
not repeat.
.store trantime=1 time=0.00001
Example 9: HSPICE does not do a store operation.
.store trantime=1
See Also
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
299
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SUBCKT
.SUBCKT
Defines a subcircuit in a netlist.
Syntax
Nodes and Parameters
.SUBCKT subnam n1 n2 n3 ... [param=val]
.ENDS
.SUBCKT SubNamePinList [SubDefaultsList]
.ENDS
Parameter String
.SUBCKT subnam n1 n2 n3 ... [param=str('string')]
.ENDS
Isomorphic Analyses
.SUBCKT analyses_sb [start=p1 stop=p2 steps=p3]
.DC …
.AC …
.TRAN …
.ENDS analyses_sb
...followed by
x1 analyses_sb [start=a1] [stop=a2] [steps=a3]
x2 analyses_sb [start=b1] [stop=b2] [steps=b3]
Argument
Description
subnam
Reference name for the subcircuit model call.
n1...
Node numbers for external reference; cannot be the ground node
(0, gnd, ground, gnd!). Any element nodes that are in the subcircuit,
but are not in this list are strictly local with three exceptions:
■
■
■
parnam
Ground node (0, gnd, ground, gnd!).
Nodes assigned using BULK=node in MOSFET or BJT models.
Nodes assigned using the .GLOBAL command.
Parameter name set to a value. Use only in the subcircuit. To
override this value, assign it in the subcircuit call or set a value in
a .PARAM command.
SubDefaultsList SubParam1=Expression [SubParam2=Expression...]
300
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SUBCKT
Argument
Description
analysis_sb
Reference name for the isomorphic analyses that can be run in a
subckt block.
p1...p2...p3
Parameters specified for the start, stop, and number of steps.
Description
Use this command to define a subcircuit in your netlist. You can create a
subcircuit description for a commonly used circuit and include one or more
references to the subcircuit in your netlist.
When you use hierarchical subcircuits, you can pick default values for circuit
elements in a .SUBCKT command. You can use this feature in cell definitions to
simulate the circuit with typical values.
The isomorphic analyses feature enables you to run unrelated analyses (.DC,
.AC, and .TRAN) many times during a simulation by grouping the set of
analyses into a subcircuit, which performs multiple analyses in one simulation
with calls to the subcircuit. The usage model is: Specify the analyses
commands within the subckt definition block and then instantiate the subckt to
perform the analyses. Each call of the subcircuit is treated as an individual
analysis with its own set of parameters.
Use the .ENDS command to terminate a .SUBCKT command.
Note:
Using -top subck_name on the command line effectively
eliminates the need for the .subckt subckt_name and
.ends subckt_name.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
301
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SUBCKT
Examples
Example 1
Defining two subcircuits: SUB1 and SUB2. These are resistor-divider
networks, whose resistance values are parameters (variables). The X1,
X2, and X3 commands call these subcircuits. Because the resistor values
are different in each call, these three calls produce different subcircuits.
*FILE SUB2.SP TEST OF SUBCIRCUITS
.OPTION LIST ACCT
V1 1 0 1
.PARAM P5=5 P2=10
.SUBCKT SUB1 1 2 P4=4
R1 1 0 P4
R2 2 0 P5
X1 1 2 SUB2 P6=7
X2 1 2 SUB2
.ENDS
*
.MACRO SUB2 1 2 P6=11
R1 1 2 P6
R2 2 0 P2
.EOM
X1 1 2 SUB1 P4=6
X2 3 4 SUB1 P6=15
X3 3 4 SUB2
*
.MODEL DA D CJA=CAJA CJP=CAJP VRB=-20
IS=7.62E-18
+ PHI=.5 EXA=.5 EXP=.33
.PARAM CAJA=2.535E-16 CAJP=2.53E-16
.END
302
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SUBCKT
Example 2
Implementing an inverter that uses a Strength parameter. By default, the
inverter can drive three devices. Enter a new value for the Strength
parameter in the element line to select larger or smaller inverters for the
application.
.SUBCKT Inv a y Strength=3
Mp1 <MosPinList> pMosMod L=1.2u
W=’Strength * 2u’
Mn1 <MosPinList> nMosMod L=1.2u
W=’Strength * 1u’
.ENDS
...
xInv0 a y0 Inv
$ Default devices: p device=6u,
$ n device=3u
xInv1 a y1 Inv Strength=5
$ p device=10u,
n device=5u
xInv2 a y2 Inv Strength=1
$ p device= 2u,
n device=1u
...
Example 3
Implementing an IBIS model (in HSPICE only) that uses string
parameters to specify the IBIS file name and IBIS model name.
* Using string parameters
.subckt IBIS vccq vss out in
+ IBIS_FILE=str('file.ibs')
+ IBIS_MODEL=str('ibis_model')
ven en 0 vcc
B1 vccq vss out in en v0dq0 vccq vss
+ file= str(IBIS_FILE) model=str(IBIS_MODEL)
.ends
Example 4
Specifying Isomorphic Analyses
.subckt analyses_sb start_dc=-25 stop_dc=25 steps_dc=5
+ steps_tran=1n stop_tran=10n
.DC TEMP start_dc stop_dc steps_dc
.TRAN steps_tran stop_tran
.ends analyses_sb
...
x1 analyses_sb start_dc=25 stop_dc=75 steps_dc=10
x2 analyses_sb steps_tran=2n
x3 analyses_sb
Example 4 specifies both .DC and .TRAN analyses within the subckt. To
invoke these analyses you can call the subckts.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
303
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SUBCKT
■
Each subckt call will perform DC and Transient analysis.
■
Parameters defined in the subcircuit calls will override the default values
specified in the subcircuit definition.
■
If parameters are not defined in the subckt calls they will take the default
values given in the subcircuit.
See Also
.ENDS
.EOM
.MACRO
.MODEL
.OPTION LIST
.PARAM (or) .PARAMETER (or) .PARAMETERS
Isomorphic Analyses in Subckt Blocks
304
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SURGE
.SURGE
Automatically detects and reports a current surge that exceeds the specified
surge tolerance in HSPICE RF.
Syntax
.SURGE surge_thresholdsurge_widthnode1 [node2 ...noden]
Argument
Description
surge_threshold
Minimum absolute surge current.
surge_width
Defines the minimum duration of a surge.
noden
Any valid node name at current or lower subcircuit level.
Description
Use this command to automatically detect and report a current surge that
exceeds the specified surge tolerance. The command reports any current
surge that is greater than surge_threshold for a duration of more than
surge_width.
Surge current is defined as the current flowing into or out of a node to the lower
subcircuit hierarchy.
Examples
In this example, the .SURGE command detects any current surge that has an
absolute amplitude of more than 1mA, and that exceeds 100ns, x(xm.x1.a),
x(xm.x2.c), and x(xn.y).
.SUBCKT sa
...
.ENDS
.SUBCKT sb
...
.ENDS
.SUBCKT sx
x1 x y sa
x2 x a sb
.ENDS
xm 1 2 sx
xn 2 a sx
.SURGE 1mA
a b
c d
x y
100ns xm.x1.a xm.x2.c xn.y
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
305
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SWEEPBLOCK
.SWEEPBLOCK
Creates a sweep whose set of values is the union of a set of linear, logarithmic,
and point sweeps in HSPICE RF.
Syntax
.SWEEPBLOCK swblocknamesweepspec [sweepspec
+ [sweepspec [...]]]
Argument
Description
swblockname
Assigns a name to SWEEPBLOCK.
sweepspec
You can specify an unlimited number of sweepspec parameters. Each
sweepspec can specify a linear, logarithmic, or point sweep by using one of the
following forms:start stop increment lin npoints start stop dec npoints start stop
oct npoints start stop poi npoints p1 p2 ...
Description
Use this command to create a sweep whose set of values is the union of a set
of linear, logarithmic, and point sweeps.
You can use this command to specify DC sweeps, parameter sweeps, AC, and
HBAC frequency sweeps, or wherever HSPICE accepts sweeps.
For additional information, see “SWEEPBLOCK in Sweep Analyses” in the
HSPICE User Guide: RF Analysis.
Examples
The following example specifies a logarithmic sweep from 1 to 1e9 with more
resolution from 1e6 to 1e7:
.sweepblock freqsweep dec 10 1 1g dec 1000 1meg 10meg
See Also
.AC
.DC
.ENV
.HB
.HBAC
.HBLSP
.HBNOISE
.HBOSC
306
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.SWEEPBLOCK
.HBXF
.PHASENOISE
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
307
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TEMP (or) .TEMPERATURE
.TEMP (or) .TEMPERATURE
Specifies the circuit temperature for an HSPICE/HSPICE RF simulation.
Syntax
.TEMP t1 [t2t3 ...]
Argument
Description
t1 t2
Temperatures in ×C at when HSPICE/HSPICE RF simulates the
circuit.
Description
Use this command to specify the circuit temperature for an HSPICE simulation.
You can use either the .TEMP command or the TEMP parameter in
the .DC, .AC, and .TRAN commands. HSPICE compares the circuit simulation
temperature against the reference temperature in the TNOM option. HSPICE
uses the difference between the circuit simulation temperature and the TNOM
reference temperature to define derating factors for component values.
HSPICE RF supports only one .TEMP command in a netlist. If you use
multiple .TEMP commands, only the last one will be used.
Note:
HSPICE allows multiple .TEMP commands in a netlist and
performs multiple DC, AC or TRAN analyses for each
temperature. Do not set the temperature to the same value
multiple times.
When you use multiple temperature values in a .TEMP
command, HSPICE RF perform multiple HB, SN, PHASENOISE,
etc. analyses for each temperature. The simulation results for the
different temperature values saved using a file naming
convention consistent with .ALTER commands.
Examples
In Example 1, the .TEMP command sets the circuit temperatures for the entire
circuit simulation. To simulate the circuit by using individual elements or model
temperatures, HSPICE/HSPICE RF uses:
308
■
Temperature as set in the .TEMP command.
■
.OPTION TNOM setting (or the TREF model parameter).
■
DTEMP element temperature.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TEMP (or) .TEMPERATURE
Example 1
.TEMP -55.0 25.0 125.0
In Example 2:
■
The .TEMP command sets the circuit simulation temperature to 100 ° C.
■
You do not specify .OPTION TNOM so it defaults to 25 ° C.
■
The temperature of the diode is 30 ° C above the circuit temperature as set
in the DTEMP parameter.
That is:
■
D1temp=100 ° C + 30 ° C=130 ° .
■
HSPICE/HSPICE RF simulates the D2 diode at 100 ° C.
■
R1 simulates at 70 ° C.
Because the diode model command specifies TREF at 60 ° C, HSPICE/
HSPICE RF derates the specified model parameters by:
■
70 ° C (130 ° C - 60 ° C) for the D1 diode.
■
40 ° C (100 ° C - 60 ° C) for the D2 diode.
■
45 ° C (70 ° C - TNOM) for the R1 resistor.
Example 2
.TEMP 100
D1 N1 N2 DMOD DTEMP=30
D2 NA NC DMOD
R1 NP NN 100 TC1=1 DTEMP=-30
.MODEL DMOD D IS=1E-15 VJ=0.6 CJA=1.2E-13
+ CJP=1.3E-14 TREF=60.0
In Example 3, parameterized .TEMP is also supported.
Example 3
.param mytemp =0
.temp '105 + 3*mytemp'
See Also
.AC
.DC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
309
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TEMP (or) .TEMPERATURE
.OPTION TNOM
.TRAN
310
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TF
.TF
Calculates DC small-signal values for transfer functions.
Syntax
.TF ov srcnam
Argument
Description
ov
Small-signal output variable.
srcnam
Small-signal input source.
Description
Use this command to calculate DC small-signal values for transfer functions
(ratio of output variable to input source). You do not need to specify .OP.
The .TF command defines small-signal output and input for DC small-signal
analysis. When you use this command, HSPICE computes:
■
DC small-signal value of the transfer function (output/input)
■
Input resistance
■
Output resistance
Examples
.TF V(5,3) VIN
.TF I(VLOAD) VIN
For the first example, HSPICE computes the ratio of V(5,3) to VIN. This is the
ratio of small-signal input resistance at VIN to the small-signal output
resistance (measured across nodes 5 and 3). If you specify more than one .TF
command in a single simulation, HSPICE runs only the last .TF command.
See Also
.DC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
311
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TITLE
.TITLE
Sets the simulation title.
Syntax
.TITLE string_of_up_to_73_characters
Or, if .TITLE is not used
string_of_up_to_80_characters
Argument Description
string
Any character string up to 73 (or 80 if .TITLE is omitted) characters long.
Description
Use this command to set the simulation title in the first line of the input file. This
line is read and used as the title of the simulation, regardless of the line’s
contents. The simulation prints the title verbatim in each section heading of the
output listing file.
To set the title you can place a .TITLE command on the first line of the netlist.
However, the .TITLE syntax is not required.
In the second form of the syntax, the string is the first line of the input file. The
first line of the input file is always the implicit title. If any command appears as
the first line in a file, simulation interprets it as a title and does not execute it.
An .ALTER command does not support using the .TITLE command. To
change a title for a .ALTER command, place the title content in the .ALTER
command itself.
Examples
.TITLE my-design_netlist
See Also
.ALTER
312
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRAN
.TRAN
Starts a transient analysis that simulates a circuit at a specific time. In HSPICE
RF you can run a parameter sweep around a single analysis, but the parameter
sweep cannot change an .OPTION value. In addition, HSPICE RF does not
support the .TRAN DATA command and only supports the data-driven syntax
for parameter sweeps (for example, .TRAN AB sweepdata=name).
Syntax
Syntax for Single-Point Analysis:
.TRAN tstep1 tstop1 [START=val] [UIC]
Syntax for Double-Point Analysis:
.TRAN tstep1 tstop1 [tstep2 tstop2]
+ [START=val] [UIC] [SWEEP var type np pstart pstop]
.TRAN tstep1 tstop1 [tstep2 tstop2]
+ [START=val] [UIC] [SWEEP var START="param_expr1"
+ STOP="param_expr2" STEP="param_expr3"]
.TRAN tstep1 tstop1 [tstep2tstop2] [START=val] [UIC]
+ [SWEEP var start_expr stop_expr step_expr]
Syntax for Multipoint Analysis:
.TRAN tstep1 tstop1 [tstep2 tstop2 ...tstepN tstopN]
+ [START=val] [UIC] [SWEEP var type np pstart pstop]
.TRAN tstep1 tstop1 [tstep2 tstop2 ...tstepN tstopN]
+ [START=val] [UIC] [SWEEP var START="param_expr1"
+ STOP="param_expr2" STEP="param_expr3"]
.TRAN tstep1 tstop1 [tstep2 tstop2 ...tstepN tstopN>
+ [START=val] [UIC]
+ [SWEEP var start_expr stop_expr step_expr]
Syntax for Data-Driven Sweep:
.TRAN DATA=datanm
.TRAN tstep1 tstop1 [tstep2 tstop2 ...tstepN tstopN]
+ [START=val] [UIC] [SWEEP DATA=datanm]
.TRAN DATA=datanm [SWEEP var type np pstart pstop]
.TRAN DATA=datanm [SWEEP var START="param_expr1"
+ STOP="param_expr2" STEP="param_expr3"]
.TRAN DATA=datanm
+ [SWEEP var start_expr stop_expr step_expr]
Syntax for Monte Carlo Analysis:
.TRAN tstep1 tstop1 [tstep2 tstop2 ...tstepN tstopN]
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
313
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRAN
+ [START=val] [UIC] [SWEEP MONTE=MCcommand]
Syntax for Optimization:
.TRAN DATA=datanm OPTIMIZE=opt_par_fun
+ RESULTS=measnames MODEL=optmod
.TRAN [DATA=filename] SWEEP OPTIMIZE=OPTxxx
+ RESULTS=ierr1 ... ierrn MODEL=optmod
Argument
Description
DATA=datanm Data name, referenced in the .TRAN command.
MONTE=
MCcommand
Where MCcommand can be any of the following:
■
■
■
■
314
val
Specifies the number of random samples to produce.
val firstrun=num
Specifies the sample number on which the simulation starts.
list num
Specifies the sample number to execute.
list(num1:num2 num3 num4:num5)
Samples from num1 to num2, sample num3, and samples from num4 to
num5 are executed (parentheses are optional).
np
Number of points or number of points per decade or octave, depending on
what keyword precedes it.
param_expr...
Expressions you specify: param_expr1...param_exprN.
pincr
Voltage, current, element, or model parameter; or any temperature
increment value. If you set the type variation, use np (number of points), not
pincr.
pstart
Starting voltage, current, or temperature; or any element or model
parameter value. If you set the type variation to POI (list of points), use a list
of parameter values, instead of pstart pstop.
pstop
Final value: voltage, current, temperature; element or model param.
START
Time when printing or plotting begins.
Caution: If you use .TRAN with a .MEASURE command, a non-zero START
time can cause incorrect .MEASURE results. Do not use non-zero START
times in .TRAN commands when you also use .MEASURE.
SWEEP
Indicates that .TRAN specifies a second sweep.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRAN
Argument
Description
tstep1...
Printing or plotting increment for printer output and the suggested
computing increment for post-processing. This argument is always a
positive value.
tstop1...
Time when a transient analysis stops incrementing by the first specified time
increment (tstep1). If another tstep-tstop pair follows, analysis continues
with a new increment. This argument is always a positive value.
UIC
If you specify the UIC parameter in the .TRAN command, HSPICE does not
calculate the initial DC operating point, but directly enters transient analysis.
When you use .TRAN UIC, the .TRAN node values (at time zero) are
determined by searching for the first value found in this order: from .IC
value, then IC parameter on an element command, then .NODESET value,
otherwise use a voltage of zero.
Note that forcing a node value of the DC operating point might not satisfy
KVL and KCL. In this event you might see activity during the initial part of
the simulation. This might happen if you use UIC and do not specify some
node values, when you specify too many (conflicting) .IC values are
specified, or when you force node values and the topology changes. Forcing
a node voltage applies a fixed equivalent voltage source during DC analysis
and transient analysis removes the voltage sources to calculate the second
and later time points.
Therefore, to correct DC convergence problems use .NODESETs (without
.TRAN UIC) liberally (when a good guess can be provided) and use .ICs
sparingly (when the exact node voltage is known).
type
Any of the following keywords:
■
■
■
■
var
DEC – decade variation.
OCT – octave variation (the value of the designated variable is eight
times its previous value).
LIN – linear variation.
POI – list of points.
Name of an independent voltage or current source, any element or model
parameter, or the TEMP keyword (indicating a temperature sweep). You can
use a source value sweep, referring to the source name (SPICE style).
However, if you specify a parameter sweep, a .DATA command, or a
temperature sweep you must choose a parameter name for the source value
and subsequently refer to it in the .TRAN command. The parameter must
not start with TEMP and should be defined in advance using the .PARAM
command.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
315
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRAN
Argument
Description
firstrun
MONTE=val value specifies the number of Monte Carlo iterations to
perform. This argument specifies the desired number of iterations. HSPICE
runs from num1 to num1+val-1.
list
Iterations at which HSPICE performs a Monte Carlo analysis. You can write
more than one number after list. The colon represents “from... to...”.
Specifying only one number makes HSPICE run at only the specified point.
OPTIMIZE
When used with .TRAN and SWEEP, this argument is either opt_par_fun or
OPTxxx for a bisection/Monte Carlo analysis in HSPICE.
Description
Use to start a transient analysis that simulates a circuit at a specific time.
For single-point analysis, the values of the tstep, tstop1, and START
arguments should obey the following rules:
For double-point analysis, the values of the tstep1, tstop1, tstep2,
tstop2, and START arguments should obey the following rules:
In double-point analysis, if tstep2 < tstop1, tstop2 < tstop1, and START
is not explicitly set, the command is interpreted as:
There can be three different “DELMAX” values involved in a .TRAN command:
■
.OPTION DELMAX (value specified with this .OPTION)
■
delmax (value that can be specified with the .TRAN command)
■
“auto” DELMAX (value that is computed automatically)
When column 4 is interpreted as delmax, this command has a higher priority
than the DELMAX option. The maximum internal timestep taken by HSPICE
during transient analysis is referred to as Δt max . Its value is normally computed
automatically based on several timestep control settings. If you wish to override
the automatically computed value, and force the maximum step size to be a
specific value, you can do so with .OPTION DELMAX, or by specifying a
delmax value with the .TRAN command. If not specified, HSPICE
automatically computes a DELMAX “auto” value, based on timestep control
factors such as FS and RMAX. (For a complete list of timestep control factors,
see Transient Control Options in the HSPICE User Guide: Simulation and
Analysis.)
For multipoint analysis, the values of the tstep1, tstop1,..., tstepN,
tstopN, and START arguments should obey the following rules:
316
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRAN
The following limitation applies for HSPICE: The ratio between tstop1 and
tstep must be tstop ≤ 1e9 • tstep . For example, .TRAN 8n 8 is permissible,
but .TRAN 0.1n 8 is not.
You can initiate a store/restore operation that creates checkpoint files
describing a running process during transient analysis; the operating system
can later reconstruct the process from the contents of this file. This function is
available in HSPICE only on Redhat Linux/SuSE Linux platforms for the current
release.
Examples
Example 1
Performs and prints the transient analysis every 1 ns for 100 ns.
.TRAN 1NS 100NS
Example 2
Performs the calculation every 0.1 ns for the first 25 ns; and then every
1 ns until 40 ns. Printing and plotting begin at 10 ns.
.TRAN .1NS 25NS 1NS 40NS START=10NS
Example 3
Does the calculation every 0.1 ns for 25 ns; and then every 1 ns for 40 ns;
and then every 2 ns until 100 ns. Printing and plotting begin at 10 ns.
.TRAN .1NS 25NS 1NS 40NS 2NS 100NS START = 10NS
Example 4 performs the calculation every 10 ns for 1 μs. This example
bypasses the initial DC operating point calculation. It uses the nodal
voltages specified in the .IC command (or by IC parameters in element
commands) to calculate the initial conditions.
.TRAN 10NS 1US UIC
Example 4
Example 5
This example increases the temperature by 10 degreesC through the
range -55 degreesC to 75 degreesC. It also performs transient analysis
for each temperature.
.TRAN 10NS 1US UIC SWEEP TEMP -55 75 10
Example 6
Analyzes each load parameter value at 1 pF, 5 pF, and 10 pF.
.TRAN 10NS 1US SWEEP load POI 3 1pf 5pf 10pf
Example 7
This example is a data-driven time sweep. It uses a data file as the sweep
input. If the parameters in the data command are controlling sources,
then a piecewise linear specification must reference them.
.TRAN data=dataname
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
317
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRAN
Example 8
Performs the calculation every 10ns for 1us from the 11th to 20th Monte
Carlo trials.
.TRAN 10NS 1US SWEEP MONTE=10 firstrun=11
Example 9
Performs the calculation every 10ns for 1us at the 10th trial, then from the
20th to the 30th trial, followed by the 35th to the 40th trial and finally at
the 50th Monte Carlo trial.
.TRAN 10NS 1US SWEEP MONTE=list(10 20:30 35:40 50)
See Also
.IC
.NODESET
.STORE
.OPTION DELMAX
Timing Analysis Using Bisection
Transient Analysis
Signal Integrity Examples for netlists using .TRAN including iotran.sp,
qa8.sp, and qabounce.sp. See also ipopt.sp for an optimization example
using .TRAN.
Behavioral Application Examples for the path to the demo file invb_op.sp
demonstrating use of .TRAN with OPTIMIZE to optimize a CMOS
macromodel inverter.
318
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRANNOISE
.TRANNOISE
RF analysis activates transient noise analysis to compute the additional noise
variables over a standard .TRAN analysis. Important: FMAX has a dramatic
effect on TRANNOISE, since it controls the amount of energy each noise
source is allowed to emit. Therefore, huge values of FMAX (like 100G) can
result in huge instantaneous noise levels. FMIN sets the low frequency limit for
flicker noise, and therefore controls the energy in flicker noise sources. You can
expect some significant differences with FMAX and FMIN changes: Noise
power will increase linearly with FMAX; Flicker noise power can scale as 1/
FMIN.
Syntax
Input Syntax—Monte Carlo Single Sample Approach
.TRANNOISE output [METHOD=MC] [SEED=val]
+ [AUTOCORRELATION=0|1|off|on]
+ [FMIN=val] [FMAX=val] [SCALE=val]
Input Syntax—Monte Carlo Multi-Sample Approach
.TRANNOISE output
+ [METHOD=MC] [SEED=val] [SAMPLES=val]
+ [AUTOCORRELATION=0|1|off|on]
+ [FMIN=val][FMAX=val][SCALE=val]
Input Syntax—SDE Approach
.TRANNOISE output METHOD=SDE
+ [AUTOCORRELATION=0|1|off|on|]
+ [TIME=(all|val)]
+ [FMIN=val] [FMAX=val] [SCALE=val]
Argument
Description
output
(Required) Output node, pair of nodes, or 2-terminal element. Noise
calculations are referenced to this node (or node pair). Specify a pair of
nodes as V(n+,n-). If you specify only one node, V(n+), then HSPICE RF
reads the second node as ground. If you specify a 2-terminal element,
the noise voltage across this element is treated as the output.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
319
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRANNOISE
Argument
Description
METHOD=
MC | SDE
Specifies Monte Carlo or SDE transient noise analysis method. The
default, or, if METHOD is not specified, is the single-sample Monte Carlo
method. Specifying METHOD=SDE is required to select the transient
noise analysis SDE method.
METHOD=MC | SDE is position independent.
AUTOCORRELATION (Optional) Used to enable the autocorrelation function calculation at the
specified output (for jitter measurements, for example).
■
■
AUTOCORRELATION=0 (OFF) - (default) Autocorrelation function is
not calculated.
AUTOCORRELATION=1 (ON) - Autocorrelation function s calculated
at the specified output.
TIME
(Optional) Used to specify additional time points (breakpoints) where
time-domain noise should be evaluated in addition to those time points
that will be evaluated as part of the normal time-stepping algorithm.Use
this parameter to force noise evaluation at important time points of
interest (such as rising/falling edges). TIME=all: (default) causes timedomain noise ONOISE values to be computed and available for output at
all time points selected by the .TRAN command time-step
algorithm.TIME=val: Specifies a single additional time point at which
time domain noise is measured. The value can be numeric or a
parameter. A .TRAN analysis at this time point will be forced. Note that
time-domain noise calculations require an accompanying .TRAN
analysis at each time point. The TIME parameter may therefore add
transient analysis time-points (breakpoints) as needed while values
given outside the range of the .TRAN command constraints are ignored.
FMIN
(Optional) Base frequency used for modeling frequency dependent noise
sources. Sets bandwidth for contributing noise sources. (Default: 1/
TSTOP) See Note below.
FMAX
(Optional) Maximum frequency used for modeling frequency dependent
noise sources. Sets bandwidth for contributing noise sources. Default: 1/
TSTEP; See Note below.
SCALE
Scale factor that can be applied to uniformly amplify the intensity of all
device noise sources to exaggerate their contributions. Default: 1.0
Description
Use to analyze time-variant noise in HSPICE RF for circuits driven with nonperiodic waveforms. The transient noise analysis requires an accompanying
320
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRANNOISE
.TRAN analysis which determines the time-sampling, matrix solutions, and
deterministic output waveforms. The .TRANNOISE command is used to
activate transient noise and to compute the additional noise variables. Note that
this is consistent with how .NOISE computes additional noise outputs when
added to an .AC analysis.
The Monte Carlo approach can capture very nonlinear noise behaviors. This is
useful, for example, when the responses of circuits with noise are known to
have non-Gaussian variations about their noise-less simulations.
For an in-depth discussion, see Transient Noise Analysis in the HSPICE User
Guide: RF Analysis.
Examples
Example 1
Generates 30 Monte Carlo noise simulations beginning with a noiseless
(index=1) simulation.
.TRANNOISE v(out) SWEEP MONTE=30
Example 2
Generates 20 Monte Carlo noise simulations starting with the seed value
(i.e., index) of 31 for the first simulation.
.TRANNOISE v(out) SWEEP MONTE=20 FIRSTRUN=31
Example 3
Generates a single noise simulation, with seed value of 50, with all noise
sources amplified by a factor of 10.
.TRANNOISE v(out) SWEEP MONTE=1 FIRSTRUN=50 SCALE=10.0
Example 4
Activates SDE noise analysis, and dumps the ONOISE output to the *.tr0
file:
.TRANNOISE v(out)
.PROBE TRANNOISE ONOISE
Example 5
Activates SDE noise analysis, placing a lower bound on flicker noise to
be 10kHz, and an upper bound on all noise power at 100MHz:
.TRANNOISE v(out) FMIN=10k FMAX=100MEG
See Also
.TRAN
.NOISE
.PTDNOISE
.OPTION MCBRIEF
.OPTION MACMOD
.OPTION MODMONTE
.OPTION MONTECON
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
321
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.TRANNOISE
.OPTION RANDGEN
.OPTION SEED
322
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.UNPROTECT or .UNPROT
.UNPROTECT or .UNPROT
Restores normal output functions previously restricted by a .PROTECT
command as part of the encryption process in HSPICE.
Syntax
.UNPROTECT
Description
Use this command to restore normal output functions previously restricted by
a .PROTECT command.
■
Any elements and models located between .PROTECT and .UNPROTECT
commands, inhibit the element and model listing from the LIST option.
■
Neither the .OPTION NODE cross-reference, nor the .OP operating point
printout list any nodes within the .PROTECT and .UNPROTECT commands.
■
The .UNPROTECT command is encrypted during the encryption process.
Caution: If you use.prot/.unprot in a library or file that is not
encrypted warnings are issued that the file is encrypted and the
file or library is treated as a “black box.”
Note:
To perform a complete bias check and print all results in the
Outputs Biaschk Report, do not use .protect/.unprotect in
the netlist for the part that is used in .biaschk. For example: If
a model definition such as model nch is contained within
.prot/.unprot commands, in the *.lis you'll see a warning
message as follows: **warning** : model nch defined
in .biaschk cannot be found in netlist--ignored
Usage Note: The .prot/.unprot feature is meant for the encryption process
and not netlist echo suppression. Netlist and model echo suppression is on by
default since HSPICE C-2009.03. For a compact and better formatted output
(*.lis) file, use .OPTION LIS_NEW
See Also
.PROTECT or .PROT
.OPTION BRIEF
.BIASCHK
.OPTION LIS_NEW
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
323
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.VARIATION
.VARIATION
Specifies global and local variations on model parameters in HSPICE.
Syntax
.Variation
Define options
Define common parameters that apply to all subblocks
.Global_Variation
Define the univariate independent random variables
Define additional random variables through
transformation
Define variations of model parameters
.End_Global_Variation
.Local_Variation
Define the univariate independent random variables
Define additional random variables through
transformation
Define variations of model parameters
.Element_Variation
Define variations of element parameters
.End_Element_Variation
.End_Local_Variation
.Spatial_Variation
Define the univariate independent random variables
Define additional random variables through
transformation
Define variations of model parameters
.End_Spatial_Variation
.End_Variation
Description
Use this command to specify global, local, and spatial variations on model
parameters, resulting from variations in materials and manufacturing. If a
Variation Block is read as part of .ALTER processing, then the contents are
treated as additive. If the same parameters are redefined, HSPICE considers
this an error.
The following are parameters and options available to the Variation Block:
■
Constant parameter—definition which can be referenced anywhere within
the Variation Block:
parameter PARAM=val
324
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.VARIATION
■
Univariate Independent Random Variable normal, uniform, and
cumulative distributions below, respectively:
parameter IVarName=N()
parameter IVarName=U()
parameter IVarName=CDF(xn,yn)
■
Transformed Random Variable
parameter TVarName=expression(IVarNameIVarName)
■
Variation Definition for Model Parameter
modelType modelName paramName=Expression_For_Sigma
■
Variation Definition for Element Parameter
modelType paramName=Expression_For_Sigma
modelType(condition) paramName=Expression_For_Sigma
■
Expression_For_Sigma
Referencing a previously defined Random Variable
perturb('expression(IVarName|TVarNameIVarName TVarName)')
absolute
perturb('expression(IVarName|TVarNameIVarName TVarName)') %
relative
Referencing a previously defined Random Variable
perturb('expression(IVarName|TVarNameIVarName TVarName)')
absolute
perturb('expression(IVarName|TVarNameIVarName TVarName)') %
relative
■
Access Function
For element parameter (for example w, l, x, y):
get_E(elementParameter)
For netlist parameter (for example .param vdd, temper):
get_P(Parameter)
■
Options: For a detailed description of the Variation Block and usage
examples, see Analyzing Variability and Using the Variation Block in the
HSPICE User Guide: Simulation and Analysis and for Variation Block
options, see Control Options and Syntax.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
325
Chapter 2: HSPICE and HSPICE RF Netlist Commands
.VEC
.VEC
Calls a digital vector file from an HSPICE/HSPICE RF netlist.
Syntax
.VEC ‘digital_vector_file’
Description
Use this command to call a digital vector file from an HSPICE netlist. A digital
vector file consists of three sections:
■
Vector Pattern Definition
■
Waveform Characteristics
■
Tabular Data
The .VEC file must be a text file. If you transfer the file between UNIX/Linux and
Windows, use text mode. See Chapter 4, Digital Vector File Commands for
more information.
Examples
This is a fragment from a netlist with a call to a digital vector file.
*file: mos2bit_v.sp - adder - 2 bit all-nand-gate binary adder
*uses digital vector input
.options post nomod
.option opts fast
*
.tran .5ns 60ns
*
.vec 'digstim.vec'
...
326
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
3
3
HSPICE and RF Netlist Simulation Control
Options
Describes the HSPICE and HSPICE RF simulation control options you can set
using various forms of the .OPTION command.
You can set HSPICE and HSPICE RF simulation control options using
the .OPTION command. This chapter provides a list of the options grouped by
usage, followed by detailed descriptions of the individual options in an
alphabetical list. Note that in many cases an option is only usable in either the
HSPICE or HSPICE RF mode of operation. In a few instances, an option has
different functionality, depending on which mode (HSPICE or HSPICE RF) has
been invoked. The description of the command notes the differences.
The control options described in this chapter fall into the following broad
categories:
■
General Control Options
■
Input/Output Controls
■
Model Analysis
■
HSPICE Analysis Options
■
HSPICE RF Analysis Options
■
Transient and AC Small Signal Analysis Options
■
Transient Control (Integration) Method Options
■
.VARIATION Block Control Options
■
.DESIGN_EXPLORATION Block Control Options
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
329
Chapter 3: HSPICE and RF Netlist Simulation Control Options
General Control Options
Notes on Default Values
The typical behavior for options is:
■
Option not specified: value is default value, typically “OFF” or 0.
■
Option specified but without value: typically turns the option “ON” or to a
value of 1.
If an option has more than two values allowed, specifying it without a value sets
it to 1, if appropriate.In most cases, options without values are allowed only for
flags that can be on or off, and specifying the option without a value turns it on.
There are a few options (such as POST), where there are more than two values
allowed, but you can still specify it without a value. Usually, you should expect it
to be 1.
Use of Example Syntax
To copy and paste proven syntax use the demonstration files shipped with your
installation of HSPICE (see Listing of Demonstration Input Files). Attempting to
copy and paste from the book or help documentation may present unexpected
results, as text used in formatting may include hidden characters, white space,
etc. for visual clarity.
HSPICE Control Options Grouped By Function
General Control Options
Netlist Parser Control
.OPTION ALTCC
.OPTION DIAGNOSTIC
(or) .OPTION DIAGNO
.OPTION NOTOP
.OPTION SEARCH
.OPTION ALTCHK
.OPTION NOELCK
.OPTION NOWARN
.OPTION WARNLIMIT
(or) .OPTION WARNLIM
.OPTION BADCHR .OPTION NOMOD
330
.OPTION PARHIER
(or) .OPTION PARHIE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Input/Output Controls
Output Listing Control
.OPTION BRIEF
.OPTION LENNAM
.OPTION NOISEMINFREQ
.OPTION PATHNUM
.OPTION CAPTAB
.OPTION LIST
.OPTION NUMDGT
.OPTION STATFL
.OPTION CO
.OPTION MCBRIEF
.OPTION OPTLST
.OPTION VFLOOR
.OPTION INGOLD
.OPTION NODE
.OPTION OPTS
.MEAS Options
.OPTION MEASFAIL
.OPTION MEASFILE
.OPTION MEASOUT
.OPTION PUTMEAS
.OPTION EM_RECOVERY
.BIASCHK Options
.OPTION BIASFILE
.OPTION BIASNODE
.OPTION BIASPARALLEL
.OPTION BIAWARN
.OPTION BIASINTERVAL
Multithreading Option
.OPTION MTTHRESH
Input/Output Controls
I/O Control Options
.OPTION D_IBIS
.OPTION MONTECON
.OPTION POST
.OPTION POSTLVL
.OPTION INTERP
.OPTION OPFILE
.OPTION POSTLVL
.OPTION POSTTOP
.OPTION ITRPRT
.OPTION PROBE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
331
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Model Analysis
Interface Control Options
.OPTION ARTIST
.OPTION CSDF
.OPTION DLENCSDF
.OPTION PSF
Model Analysis
.OPTION APPENDALL
.OPTION DEFAS
.OPTION DEFPS
.OPTION NCWARN
.OPTION ASPEC
.OPTION DEFL
.OPTION DEFSA
.OPTION SOIQ0
.OPTION BSIM4PDS
.OPTION DEFNRD
.OPTION DEFSB
.OPTION WL
.OPTION DCAP
.OPTION DEFNRS
.OPTION DEFSD
.OPTION WNFLAG
.OPTION DEFAD
.OPTION DEFPD
.OPTION DEFW
Custom Models
.OPTION CMIFLAG
.OPTION CMIUSRFLAG
.OPTION CUSTCMI
Model Control
.OPTION HIER_SCALE
.OPTION MACMOD
.OPTION MODMONTE
.OPTION SEED
Scaling
.OPTION SCALE
.OPTION SCALM
Temperature
.OPTION TNOM
.OPTION XDTEMP
Resistance
.OPTION RESMIN
332
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Model Analysis
Verilog-A
.OPTION SPMODEL
.OPTION VAMODEL
Diode and BJT
.OPTION DCAP
.OPTION EXPLI
Inductor and Mutual Inductors
.OPTION GENK
.OPTION KLIM
Back Annotation Post-Layout Options
.OPTION BA_ACTIVE
.OPTION
BA_DPFPFX
.OPTION
BA_GEOSHRINK
.OPTION
BA_NETFMT
.OPTION
BA_ACTIVEHIER
.OPTION BA_ERROR
.OPTION
BA_HIERDELIM
.OPTION BA_PRINT
.OPTION
BA_ADDPARAM
.OPTION BA_FILE
.OPTION
BA_IDEALPFX
.OPTION BA_SCALE
.OPTION
BA_COUPLING
.OPTION
BA_FINGERDELIM
.OPTION
BA_MERGEPORT
.OPTION
BA_TERMINAL
RC Reduction
.OPTION LA_FREQ
.OPTION LA_MINC
.OPTION LA_MAXR
.OPTION LA_TIME
.OPTION LA_TOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
.OPTION SIM_LA
333
Chapter 3: HSPICE and RF Netlist Simulation Control Options
HSPICE Analysis Options
HSPICE Analysis Options
Transient and AC Small Signal Analysis Options
Transient Control (Integration) Method Options
.OPTION LVLTIM
.OPTION MAXORD
.OPTION METHOD
.OPTION MU
.OPTION PURETP
Transient Control Limit Options
.OPTION AUTOSTOP (or) .OPTION AUTOST
.OPTION GMIN
.OPTION ITL4
.OPTION RMAX
Error Tolerance
.OPTION ABSH
.OPTION CHGTOL
.OPTION RELH
.OPTION RELVDC
.OPTION ABSV
.OPTION EM_RECOVERY
.OPTION RELQ
.OPTION TRTOL
.OPTION ABSVAR
.OPTION KCLTEST
.OPTION RELV
.OPTION VNTOL
.OPTION ABSVDC
.OPTION MAXAMP
Speed and Accuracy
.OPTION BDFATOL
.OPTION DVDT
.OPTION IMAX
.OPTION RISETIME
(or) .OPTION RISETI
.OPTION BDFRTOL
.OPTION DVTR
.OPTION IMIN
.OPTION RMIN
.OPTION CSHUNT
.OPTION FAST
.OPTION ITL3
.OPTION RUNLVL
.OPTION CVTOL
.OPTION FS
.OPTION ITL4
.OPTION SLOPETOL
.OPTION DELMAX
.OPTION FT
.OPTION ITL5
.OPTION TIMERES
.OPTION DI
.OPTION GMIN
.OPTION NEWTOL
.OPTION TRCON
334
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient and AC Small Signal Analysis Options
Bypass
.OPTION BYPASS
.OPTION BYTOL
.OPTION MBYPASS
AC/Noise
.OPTION NOISEMINFREQ
Spectral Analysis Controls
.OPTION FFT_ACCURATE
.OPTION FFTOUT
Transmission Lines
.OPTION RISETIME (or) .OPTION RISETI
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
.OPTION WACC
335
Chapter 3: HSPICE and RF Netlist Simulation Control Options
HB Options
HSPICE RF Analysis Options
HB Options
.OPTION HBACKRYLOVDIM
.OPTION HBKRYLOVDIM
.OPTION HBTOL
.OPTION
HBACKRYLOVITER (or)
HBAC_KRYLOV_ITER
.OPTION HBKRYLOVMAXITER
(or) HB_KRYLOV_MAXITER
.OPTION
HBTRANFREQSEARCH
.OPTION HBACTOL
.OPTION HBKRYLOVTOL
.OPTION HBTRANINIT
.OPTION HBCONTINUE
.OPTION HBLINESEARCHFAC
.OPTION HBTRANPTS
.OPTION HBFREQABSTOL
.OPTION HBMAXITER (or)
HB_MAXITER
.OPTION HBTRANSTEP
.OPTION HBFREQRELTOL
.OPTION HBOSCMAXITER (or)
HBOSC_MAXITER
.OPTION LOADHB
.OPTION HB_GIBBS
.OPTION HBPROBETOL
.OPTION SAVEHB
.OPTION HBJREUSE
.OPTION HBSOLVER
.OPTION TRANFORHB
.OPTION HBJREUSETOL
Phase Noise Analysis
.OPTION BPNMATCHTOL
.OPTION
PHASENOISEKRYLOVITER
(or)
PHASENOISE_KRYLOV_ITER
.OPTION PHNOISELORENTZ
.OPTION
PHASENOISEKRYLOVDIM
.OPTION PHASENOISETOL
.OPTION PHNOISEAMPM
336
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Power Analysis
Power Analysis
.OPTION
SIM_POWER_ANALYSIS
.OPTION
SIM_POWERDC_HSPICE
.OPTION
SIM_POWERSTOP
.OPTION SIM_POWER_TOP
.OPTION SIM_POWERPOST
.OPTION
SIM_POWERDC_ACCURACY
.OPTION SIM_POWERSTART
RC Network Reduction
.OPTION SIM_LA
.OPTION SIM_LA_MAXR
.OPTION SIM_LA_TOL
.OPTION SIM_LA_FREQ
.OPTION SIM_LA_MINC
.OPTION SIM_LA_TIME
Simulation Output
.OPTION SIM_POSTAT
.OPTION SIM_POSTSCOPE
.OPTION SIM_POSTDOWN
.OPTION SIM_POSTSKIP
.OPTION SIM_POSTTOP
Shooting Newton Options
.OPTION
LOADSNINIT
.OPTION
SAVESNINIT
.OPTION
SNACCURACY
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
.OPTION
SNMAXITER (or)
SN_MAXITER
337
Chapter 3: HSPICE and RF Netlist Simulation Control Options
DSPF Options
DSPF Options
.OPTION SIM_DELTAI
.OPTION SIM_DSPF_INSERROR
.OPTION
SIM_DSPF_SCALEC
.OPTION SIM_DELTAV
.OPTION SIM_DSPF_LUMPCAPS
.OPTION
SIM_DSPF_SCALER
.OPTION SIM_DSPF
.OPTION SIM_DSPF_MAX_ITER
.OPTION
SIM_DSPF_VTOL
.OPTION SIM_DSPF_ACTIVE
.OPTION SIM_DSPF_RAIL
SPEF Options
.OPTION SIM_SPEF
.OPTION
SIM_SPEF_MAX_ITER
.OPTION
SIM_SPEF_SCALER
.OPTION SIM_SPEF_ACTIVE
.OPTION
SIM_SPEF_PARVALUE
.OPTION
SIM_SPEF_VTOL
.OPTION SIM_SPEF_INSERROR
.OPTION SIM_SPEF_RAIL
.OPTION
SIM_SPEF_LUMPCAPS
.OPTION SIM_SPEF_SCALEC
Transient Accuracy Options
338
.OPTION FFT_ACCURATE
.OPTION SIM_ORDER
.OPTION SIM_TRAP
.OPTION SIM_ACCURACY
.OPTION SIM_TG_THETA
.OPTION
SIM_OSC_DETECT_TOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
Alphabetical Listing of HSPICE Control Options
The following is the alphabetical list of links to the HSPICE/RF control option
set. For commands see HSPICE and HSPICE RF Netlist Commands.
■
.OPTION ABSH
■
.OPTION ABSI
■
.OPTION ABSIN
■
.OPTION ABSMOS
■
.OPTION ABSTOL
■
.OPTION ABSV
■
.OPTION ABSVAR
■
.OPTION ABSVDC
■
.OPTION ACCURATE
■
.OPTION ACOUT
■
.OPTION ALTCC
■
.OPTION ALTCHK
■
.OPTION APPENDALL
■
.OPTION ARTIST
■
.OPTION ASPEC
■
.OPTION AUTOSTOP (or) .OPTION AUTOST
■
.OPTION BA_ACTIVE
■
.OPTION BA_ACTIVEHIER
■
.OPTION BA_ADDPARAM
■
.OPTION BA_COUPLING
■
.OPTION BA_DPFPFX
■
.OPTION BA_ERROR
■
.OPTION BA_FILE
■
.OPTION BA_FINGERDELIM
■
.OPTION BA_GEOSHRINK
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
339
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
340
■
.OPTION BA_HIERDELIM
■
.OPTION BA_IDEALPFX
■
.OPTION BA_MERGEPORT
■
.OPTION BA_NETFMT
■
.OPTION BA_PRINT
■
.OPTION BA_SCALE
■
.OPTION BA_TERMINAL
■
.OPTION BADCHR
■
.OPTION BDFATOL
■
.OPTION BDFRTOL
■
.OPTION BEEP
■
.OPTION BIASFILE
■
.OPTION BIASINTERVAL
■
.OPTION BIASNODE
■
.OPTION BIASPARALLEL
■
.OPTION BIAWARN
■
.OPTION BINPRNT
■
.OPTION BPNMATCHTOL
■
.OPTION BRIEF
■
.OPTION BSIM4PDS
■
.OPTION BYPASS
■
.OPTION BYTOL
■
.OPTION CAPTAB
■
.OPTION CFLFLAG
■
.OPTION CHGTOL
■
.OPTION CMIMCFLAG
■
.OPTION CMIFLAG
■
.OPTION CMIPATH
■
.OPTION CMIUSRFLAG
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
■
.OPTION CONVERGE
■
.OPTION CPTIME
■
.OPTION CSCAL
■
.OPTION CSDF
■
.OPTION CSHDC
■
.OPTION CSHUNT
■
.OPTION CUSTCMI
■
.OPTION CVTOL
■
.OPTION D_IBIS
■
.OPTION DCAP
■
.OPTION DCCAP
■
.OPTION DCFOR
■
.OPTION DCHOLD
■
.OPTION DCIC
■
.OPTION DCON
■
.OPTION DCSTEP
■
.OPTION DCTRAN
■
.OPTION DEFAD
■
.OPTION DEFAS
■
.OPTION DEFL
■
.OPTION DEFNRD
■
.OPTION DEFNRS
■
.OPTION DEFPD
■
.OPTION DEFPS
■
.OPTION DEFSA
■
.OPTION DEFSB
■
.OPTION DEFSD
■
.OPTION DEFW
■
.OPTION DEGF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
341
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
342
■
.OPTION DEGFN
■
.OPTION DEGFP
■
.OPTION DELMAX
■
.OPTION DI
■
.OPTION DIAGNOSTIC (or) .OPTION DIAGNO
■
.OPTION DLENCSDF
■
.OPTION DV
■
.OPTION DVDT
■
.OPTION DVTR
■
.OPTION DYNACC
■
.OPTION EM_RECOVERY
■
.OPTION EPSMIN
■
.OPTION EXPLI
■
.OPTION EXPMAX
■
.OPTION FAST
■
.OPTION FFT_ACCURATE
■
.OPTION FFTOUT
■
.OPTION FMAX
■
.OPTION FS
■
.OPTION FSCAL
■
.OPTION FT
■
.OPTION GDCPATH
■
.OPTION GENK
■
.OPTION GEOSHRINK
■
.OPTION GMAX
■
.OPTION GMIN
■
.OPTION GMINDC
■
.OPTION GRAMP
■
.OPTION GSCAL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
■
.OPTION GSHDC
■
.OPTION GSHUNT
■
.OPTION HBACKRYLOVDIM
■
.OPTION HBACKRYLOVITER (or) HBAC_KRYLOV_ITER
■
.OPTION HBACTOL
■
.OPTION HBCONTINUE
■
.OPTION HBFREQABSTOL
■
.OPTION HBFREQRELTOL
■
.OPTION HB_GIBBS
■
.OPTION HBJREUSE
■
.OPTION HBJREUSETOL
■
.OPTION HBKRYLOVDIM
■
.OPTION HBKRYLOVTOL
■
.OPTION HBKRYLOVMAXITER (or) HB_KRYLOV_MAXITER
■
.OPTION HBLINESEARCHFAC
■
.OPTION HBMAXITER (or) HB_MAXITER
■
.OPTION HBOSCMAXITER (or) HBOSC_MAXITER
■
.OPTION HBPROBETOL
■
.OPTION HBSOLVER
■
.OPTION HBTOL
■
.OPTION HBTRANFREQSEARCH
■
.OPTION HBTRANINIT
■
.OPTION HBTRANPTS
■
.OPTION HBTRANSTEP
■
.OPTION HIER_DELIM
■
.OPTION HIER_SCALE
■
.OPTION IC_ACCURATE
■
.OPTION ICSWEEP
■
.OPTION IMAX
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
343
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
344
■
.OPTION IMIN
■
.OPTION INGOLD
■
.OPTION INTERP
■
.OPTION IPROP
■
.OPTION ITL1
■
.OPTION ITL2
■
.OPTION ITL3
■
.OPTION ITL4
■
.OPTION ITL5
■
.OPTION ITLPTRAN
■
.OPTION ITLPZ
■
.OPTION ITRPRT
■
.OPTION IVTH
■
.OPTION KCLTEST
■
.OPTION KLIM
■
.OPTION LA_FREQ
■
.OPTION LA_MAXR
■
.OPTION LA_MINC
■
.OPTION LA_TIME
■
.OPTION LA_TOL
■
.OPTION LENNAM
■
.OPTION LIMPTS
■
.OPTION LIMTIM
■
.OPTION LISLVL
■
.OPTION LIS_NEW
■
.OPTION LIST
■
.OPTION LOADHB
■
.OPTION LOADSNINIT
■
.OPTION LSCAL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
■
.OPTION LVLTIM
■
.OPTION MACMOD
■
.OPTION MAXAMP
■
.OPTION MAXORD
■
.OPTION MAXWARNS
■
.OPTION MBYPASS
■
.OPTION MCBRIEF
■
.OPTION MEASDGT
■
.OPTION MEASFAIL
■
.OPTION MEASFILE
■
.OPTION MEASFORM
■
.OPTION MEASOUT
■
.OPTION MESSAGE_LIMIT
■
.OPTION METHOD
■
.OPTION MODMONTE
■
.OPTION MODPRT
■
.OPTION MONTECON
■
.OPTION MOSRALIFE
■
.OPTION MOSRASORT
■
.OPTION MRAAPI
■
.OPTION MRAEXT
■
.OPTION MRAPAGED
■
.OPTION MRA00PATH, MRA01PATH, MRA02PATH, MRA03PATH
■
.OPTION MTTHRESH
■
.OPTION MU
■
.OPTION NCFILTER
■
.OPTION NCWARN
■
.OPTION NEWTOL
■
.OPTION NODE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
345
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
346
■
.OPTION NOELCK
■
.OPTION NOISEMINFREQ
■
.OPTION NOMOD
■
.OPTION NOPIV
■
.OPTION NOTOP
■
.OPTION NOWARN
■
.OPTION NUMDGT
■
.OPTION NUMERICAL_DERIVATIVES
■
.OPTION NXX
■
.OPTION OFF
■
.OPTION OPFILE
■
.OPTION OPTCON
■
.OPTION OPTLST
■
.OPTION OPTPARHIER
■
.OPTION OPTS
■
.OPTION PARHIER (or) .OPTION PARHIE
■
.OPTION PATHNUM
■
.OPTION PCB_SCALE_FORMAT
■
.OPTION PHASENOISEKRYLOVDIM
■
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER
■
.OPTION PHASENOISETOL
■
.OPTION PHASETOLI
■
.OPTION PHASETOLV
■
.OPTION PHD
■
.OPTION PHNOISELORENTZ
■
.OPTION PHNOISEAMPM
■
.OPTION PIVOT
■
.OPTION PIVTOL
■
.OPTION POST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
■
.OPTION POSTLVL
■
.OPTION POST_VERSION
■
.OPTION POSTTOP
■
.OPTION PROBE
■
.OPTION PSF
■
.OPTION PURETP
■
.OPTION PUTMEAS
■
.OPTION PZABS
■
.OPTION PZTOL
■
.OPTION RADEGFILE
■
.OPTION RADEGOUTPUT
■
.OPTION RANDGEN
■
.OPTION REDEFSUB
■
.OPTION RELH
■
.OPTION RELI
■
.OPTION RELIN
■
.OPTION RELMOS
■
.OPTION RELQ
■
.OPTION RELTOL
■
.OPTION RELV
■
.OPTION RELVAR
■
.OPTION RELVDC
■
.OPTION REPLICATES
■
.OPTION RES_BITS
■
.OPTION RESMIN
■
.OPTION RISETIME (or) .OPTION RISETI
■
.OPTION RITOL
■
.OPTION RMAX
■
.OPTION RMIN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
347
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
348
■
.OPTION RUNLVL
■
.OPTION SAMPLING_METHOD
■
.OPTION SAVEHB
■
.OPTION SAVESNINIT
■
.OPTION SCALE
■
.OPTION SCALM
■
.OPTION SEARCH
■
.OPTION SEED
■
.OPTION SHRINK
■
.OPTION SIM_ACCURACY
■
.OPTION SIM_DELTAI
■
.OPTION SIM_DELTAV
■
.OPTION SIM_DSPF
■
.OPTION SIM_DSPF_ACTIVE
■
.OPTION SIM_DSPF_INSERROR
■
.OPTION SIM_DSPF_LUMPCAPS
■
.OPTION SIM_DSPF_MAX_ITER
■
.OPTION SIM_DSPF_RAIL
■
.OPTION SIM_DSPF_SCALEC
■
.OPTION SIM_DSPF_SCALER
■
.OPTION SIM_DSPF_VTOL
■
.OPTION SIM_LA
■
.OPTION SIM_LA_FREQ
■
.OPTION SIM_LA_MAXR
■
.OPTION SIM_LA_MINC
■
.OPTION SIM_LA_TIME
■
.OPTION SIM_LA_TOL
■
.OPTION SIM_ORDER
■
.OPTION SIM_OSC_DETECT_TOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
■
.OPTION SIM_POSTAT
■
.OPTION SIM_POSTDOWN
■
.OPTION SIM_POSTSCOPE
■
.OPTION SIM_POSTSKIP
■
.OPTION SIM_POSTTOP
■
.OPTION SIM_POWER_ANALYSIS
■
.OPTION SIM_POWER_TOP
■
.OPTION SIM_POWERDC_ACCURACY
■
.OPTION SIM_POWERDC_HSPICE
■
.OPTION SIM_POWERPOST
■
.OPTION SIM_POWERSTART
■
.OPTION SIM_POWERSTOP
■
.OPTION SIM_SPEF
■
.OPTION SIM_SPEF_ACTIVE
■
.OPTION SIM_SPEF_INSERROR
■
.OPTION SIM_SPEF_LUMPCAPS
■
.OPTION SIM_SPEF_MAX_ITER
■
.OPTION SIM_SPEF_PARVALUE
■
.OPTION SIM_SPEF_RAIL
■
.OPTION SIM_SPEF_SCALEC
■
.OPTION SIM_SPEF_SCALER
■
.OPTION SIM_SPEF_VTOL
■
.OPTION SIM_TG_THETA
■
.OPTION SIM_TRAP
■
.OPTION SI_SCALE_SYMBOLS
■
.OPTION SLOPETOL
■
.OPTION SNACCURACY
■
.OPTION SNCONTINUE
■
.OPTION SNMAXITER (or) SN_MAXITER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
349
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
350
■
.OPTION SOIQ0
■
.OPTION SPLIT_DP
■
.OPTION SPMODEL
■
.OPTION STATFL
■
.OPTION STRICT_CHECK
■
.OPTION SX_FACTOR
■
.OPTION SYMB
■
.OPTION TIMERES
■
.OPTION TMIFLAG
■
.OPTION TMIPATH
■
.OPTION TMIVERSION
■
.OPTION TNOM
■
.OPTION TRANFORHB
■
.OPTION TRCON
■
.OPTION TRTOL
■
.OPTION UNWRAP
■
.OPTION VAMODEL
■
.OPTION VERIFY
■
.OPTION VFLOOR
■
.OPTION VNTOL
■
.OPTION WACC
■
.OPTION WARN
■
.OPTION WARN_SEP
■
.OPTION WARNLIMIT (or) .OPTION WARNLIM
■
.OPTION WAVE_POP
■
.OPTION WDELAYOPT
■
.OPTION WDF
■
.OPTION WINCLUDEGDIMAG
■
.OPTION WL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
Transient Accuracy Options
■
.OPTION WNFLAG
■
.OPTION XDTEMP
■
.OPTION (X0R,X0I)
■
.OPTION (X1R,X1I)
■
.OPTION (X2R,X21)
■
.VARIATION Block Control Options
■
.DESIGN_EXPLORATION Block Control Options
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
351
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSH
.OPTION ABSH
Sets the absolute current change through voltage-defined branches.
Syntax
.OPTION ABSH=x
Default
0.0
Description
Use this option to set the absolute current change through voltage-defined
branches (voltage sources and inductors). Use this option with options DI and
RELH to check for current convergence.
See Also
.OPTION DI
.OPTION RELH
352
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSI
.OPTION ABSI
Sets the absolute error tolerance for branch currents in diodes, BJTs, and
JFETs during DC and transient analysis.
Syntax
.OPTION ABSI=x
Default
1e-9 when KCLTEST=0 or 1e-6 when KCLTEST=1.
Description
Use this option to set the absolute error tolerance for branch currents in diodes,
BJTs, and JFETs during DC and transient analysis. Decrease ABSI if accuracy
is more important than convergence time.
To analyze currents less than 1 nanoamp, change ABSI to a value at least two
orders of magnitude smaller than the minimum expected current. Min value: 1e25; Max value: 10.
See Also
.AC
.OPTION ABSMOS
.OPTION KCLTEST
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
353
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSIN
.OPTION ABSIN
Convergence criteria for bisection/passfail optimization.
Syntax
.OPTION ABSIN=val
Default
None
Description
This option invokes the absolute input parameter value and takes effect only for
bisection methods bisection or passfail. When set as .OPTION ABSIN,
it overrides all optimization model card accuracy settings and ignores the
relout and itropt parameters; when set in the model card, absin takes
effect only for the specified model. In cases where both absin and relin are
set, absin takes higher priority and dominates the simulation.
Examples
.OPTION ABSIN=5.0e-11
For use in a model card:
.MODEL optmod opt absin=5.0e-11
See Also
.MODEL
354
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSMOS
.OPTION ABSMOS
Specifies the current error tolerance for MOSFET devices in DC or transient
analysis.
Syntax
.OPTION ABSMOS=x
Default
1uA
Description
Use this option to specify the current error tolerance for MOSFET devices in
DC or transient analysis. The ABSMOS setting determines whether the drain-tosource current solution has converged. The drain-to-source current converged
if:
■
The difference between the drain-to-source current in the last iteration and
the current iteration is less than ABSMOS, or
■
This difference is greater than ABSMOS, but the percent change is less than
RELMOS.
Min value: 1e-15; Max value 10.
If other accuracy tolerances also indicate convergence, HSPICE solves the
circuit at that timepoint and calculates the next timepoint solution. For lowpower circuits, optimization, and single transistor simulations, set ABSMOS=1e12.
See Also
.DC
.OPTION RELMOS
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
355
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSTOL
.OPTION ABSTOL
Sets the absolute error tolerance for branch currents in DC and transient
analysis.
Syntax
.OPTION ABSTOL=x
Default
1e-9
Description
Use this option to set the absolute error tolerance for branch currents in DC and
transient analysis. Decrease ABSTOL if accuracy is more important than
convergence time. ABSTOL is the same as ABSI. Min value: 1e-25; Max value:
10.
See Also
.DC
.OPTION ABSI
.OPTION ABSMOS
.TRAN
356
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSV
.OPTION ABSV
Sets the absolute minimum voltage for DC and transient analysis.
Syntax
.OPTION ABSV=x
Default
50 uV
Description
Use this option to set the absolute minimum voltage for DC and transient
analysis.ABSV is the same as VNTOL.
■
If accuracy is more critical than convergence, decrease ABSV.
■
If you need voltages less than 50 uV, reduce ABSV to two orders of
magnitude less than the smallest desired voltage. This ensures at least two
significant digits.
Typically, you do not need to change ABSV, except to simulate a high-voltage
circuit. A reasonable value for 1000-volt circuits is 5 to 50 uV. Default value: 5e05; Min value: 0; Max value: 10.
See Also
.DC
.OPTION VNTOL
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
357
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSVAR
.OPTION ABSVAR
Sets the absolute limit for maximum voltage change between time points.
Syntax
.OPTION ABSVAR=volts
Default
0.5 (volts)
Description
Use this option to set the absolute limit for the maximum voltage change from
one time point to the next. Use this option with .OPTION DVDT. If the simulator
produces a convergent solution that is greater than ABSVAR, HSPICE discards
the solution, sets the timestep to a smaller value and recalculates the solution.
This is called a timestep reversal.
For additional information, see “DVDT Dynamic Timestep” in the HSPICE User
Guide: Simulation and Analysis.
See Also
.OPTION DVDT
358
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ABSVDC
.OPTION ABSVDC
Sets the minimum voltage for DC and transient analysis.
Syntax
.OPTION ABSVDC=volts
Default
50uV.
Description
Use this option to set the minimum voltage for DC and transient analysis. If
accuracy is more critical than convergence, decrease ABSVDC. If you need
voltages less than 50 uV, reduce ABSVDC to two orders of magnitude less than
the smallest voltage. This ensures at least two digits of significance. Typically,
you do not need to change ABSVDC unless you simulate a high-voltage circuit.
For 1000-volt circuits, a reasonable value is 5 to 50 uV.
See Also
.DC
.OPTION VNTOL
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
359
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ACCURATE
.OPTION ACCURATE
Selects a time algorithm for circuits such as high-gain comparators.
Syntax
.OPTION ACCURATE=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to select a time algorithm that uses LVLTIM=3 and DVDT=2 for
circuits such as high-gain comparators. Use this option with circuits that
combine high gain and large dynamic range to guarantee accurate solutions in
HSPICE. When set to 1, this option sets these control options:
The default does not set the above control options.
In HSPICE RF, this option turns on .OPTION FFT_ACCURATE and is
subordinate to .OPTION SIM_ACCURACY.
To see how use of the ACCURATE option impacts the value settings when
used with .METHOD=GEAR, and other options, see Appendix B, How Options
Affect other Options.
See Also
.OPTION ABSVAR
.OPTION DVDT
.OPTION FFT_ACCURATE
.OPTION FT
.OPTION LVLTIM
.OPTION METHOD
.OPTION RELMOS
.OPTION RELVAR
.OPTION SIM_ACCURACY
360
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ACOUT
.OPTION ACOUT
Specifies the method for calculating differences in AC output values.
Syntax
.OPTION ACOUT=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to specify a method for calculating the differences in AC output
values for magnitude, phase, and decibels for print output and plots.
■
ACOUT=0: selects the SPICE method which calculates the magnitude of the
differences real and imaginary in HSPICE. (Rarely used, but available for
backward compatability.)
■
ACOUT=1: (rarely used by analog and HSPICE RF designers) selects the
HSPICE method which calculates the difference of the magnitudes of the
values real and imaginary.
Examples
ACOUT=0
VR(N1,N2) = REAL [V(N1,0) - V(N2,0)]
VI(N1,N2) = IMAG [V(N1,0) - V(N2,0)]
Magnitude
VM(N1,N2) = [VR(N1,N2)^2+VI(N1,N2)^2]0.5 Phase
VP(N1,N2) = ARCTAN[VI(N1,N2)/VR(N1,N2)]
Decibel
VDB(N1,N2) = 20 * LOG10[VM(N1,N2)]
ACOUT=1
VR(N1,N2) = REAL [V(N1,0)] - REAL [V(N2,0)]
VI(N1,N2) = IMAG [V(N1,0)] - IMAG [V(N2,0)] Magnitude
VM(N1,0) = [VR(N1,0)^2 + VI(N1,0)^2]0.5
VM(N2,0) = [VR(N2,0)^2 + VI(N2,0)^2]0.5
VM(N1,N2) = VM(N1,0) - VM(N2,0)
Phase
VP(N1,0) = ARCTAN[VI(N1,0)/VR(N1,0)]
VP(N2,0) = ARCTAN[VI(N2,0)/VR(N2,0)]VP(N1,N2) = VP(N1,0) VP(N2,0)
Decibel
VDB(N1,N2) = 20 * LOG10(VM(N1,0)/VM(N2,0))
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
361
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ALTCC
.OPTION ALTCC
Sets onetime reading of the input netlist for multiple .ALTER commands.
Syntax
.OPTION ALTCC=[-1|0|1]
Default
0
Description
Use this option to enable HSPICE to read the input netlist only once for multiple
.ALTER commands.
■
ALTCC=1 reads input netlist only once for multiple .ALTER commands.
■
ALTCC=0 or -1 disables this option. HSPICE does not output a warning
message during transient analysis. Results are output following analysis.
.OPTION ALTCC or .OPTION ALTCC=1 ignores parsing of an input netlist
before an .ALTER command during standard cell library characterization only
when an .ALTER command changes parameters, source stimulus, analysis, or
passive elements. Otherwise, this option is ignored.
See Also
.ALTER
.LIB
362
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ALTCHK
.OPTION ALTCHK
Disables (or re-enables) topology checking in redefined elements (in altered
netlists).
Syntax
.OPTION ALTCHK=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
By default, HSPICE automatically reports topology errors in the latest elements
in your top-level netlist. It does not report errors in elements that you redefine
by using the .ALTER command (altered netlist).
To enable topology checking redefined elements in the .ALTER block, set:
.OPTION ALTCHK=1or .OPTION ALTCHK
To disable topology checking in redefined elements (that is, to check topology
only in the top-level netlist, not in the altered netlist), set:
.OPTION ALTCHK=0
See Also
.ALTER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
363
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION APPENDALL
.OPTION APPENDALL
Allows the top hierarchical level to use the .APPENDMODEL command even if
the MOSFET model is embedded in a subcircuit.
Syntax
.OPTION APPENDALL
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option when, for example, MOSFET model cards from fabs might be
embedded in subcircuit definitions. The option ends the need to edit fab model
files to include .APPENDMODEL commands in subcircuit definitions.When this
option is declared above the .APPENDMODEL command, then the main
(uppermost) circuit level hierarchy can be used, even if the MOSFET model is
embedded in a subcircuit. With this option, if the .APPENDMODEL command
appears both in the main circuit and in a subcircuit, the .APPENDMODEL in the
subcircuit takes priority.Without this option, the rules of .APPENDMODEL remain
unchanged.
Examples
In this example, the .APPENDMODEL in the main circuit is used.
.option appendall
.appendmodel n_ra mosra nch nmos
.SUBCKT mosra_test 1 2 3 4
M1 1 2 3 4 nch L=PL W=PW
.model nch nmos level= ...
.ENDS
In this example, the .APPENDMODEL in the subcircuit is used.
.option appendall
.appendmodel n_ra mosra nch nmos
.SUBCKT mosra_test 1 2 3 4
M1 1 2 3 4 nch L=PL W=PW
.model nch nmos level= ...
.appendmodel n_ra1 mosra nch nmos
.ENDS
See Also
.APPENDMODEL
364
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION APPENDALL
.MODEL
.MOSRA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
365
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ARTIST
.OPTION ARTIST
Enables the CadenceTM Virtuoso® Analog Design Environment interface.
Syntax
.OPTION ARTIST=[0|1|2]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 2
Description
Enables the Virtuoso® Analog Design Environment if ARTIST=2. This option
requires a specific license. For HSPICE RF, this option allows you to include
HSPICE RF analyses such as Harmonic Balance, Shooting Newton, and their
associated small-signal analyses and use their native waveform viewer.
This option is generally used together with .OPTION PSF. If you use .OPTION
PSF=1 or 2 with ARTIST=1 or 2 then the output format is always binary
(Parameter Storage Format) and you need to use the Cadence ADE converter
utility to change the binary format to ASCII format.
Note:
The PSF format is only supported on Sun/SPARC, Red Hat/
SUSE Linux and IBM AIX platforms as well as the 64-bit
versions.
The syntax is:
ADE_install_dir/platform/tools/dfII/bin/psf -i input_file
-o output_file
See Also
.OPTION PSF
366
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ASPEC
.OPTION ASPEC
Sets HSPICE or HSPICE RF to ASPEC-compatibility mode.
Syntax
.OPTION ASPEC=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to set the application to ASPEC-compatibility mode. When you
set this option to 1, the simulator reads ASPEC models and netlists, and the
results are compatible.
If you set ASPEC, the following model parameters default to ASPEC values:
■
ACM=1: Changes the default values for CJ, IS, NSUB, TOX, U0, and UTRA.
■
Diode Model: TLEV=1 affects temperature compensation for PB.
■
MOSFET Model: TLEV=1 affects PB, PHB, VTO, and PHI.
■
SCALM, SCALE: Sets the model scale factor to microns for length
dimensions.
■
WL: Reverses implicit order for stating width and length in a MOSFET
command. The default (WL=0) assigns the length first, then the width.
See Also
.OPTION SCALE
.OPTION SCALM
.OPTION WL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
367
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION AUTOSTOP (or) .OPTION AUTOST
.OPTION AUTOSTOP (or) .OPTION AUTOST
Stops a transient analysis in HSPICE or HSPICE RF after calculating all TRIGTARG, FIND-WHEN, and FROM-TO measure functions.
Syntax
.OPTION AUTOSTOP
-or.OPTION AUTOSTOP=’expression’
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to terminate a transient analysis in HSPICE after calculating all
TRIG-TARG, FIND-WHEN, and FROM-TO measure functions. This option can
substantially reduce CPU time. You can use the AUTOSTOP option with any
measure type. You can also use the result of the preceding measurement as
the next measured parameter.
When using .OPTION AUTOSTOP=’expression’, the ‘expression’ can only
involve measure results, a logical AND (&&) or a logical OR(||). Using these
types of expressions ends the simulation if any one of a set of .MEASURE
commands succeeds, even if the others are not completed.
Also terminates the simulation after completing all .MEASURE commands. This
is of special interest when testing corners.
Examples
.option autostop='m1&&m2||m4'
.meas tran m1 trig v(bd_a0) val='ddv/2'
+ val='ddv/2' rise=1
.meas tran m2 trig v(bd_a0) val='ddv/2'
+ val='ddv/2' rise=2
.meas tran m3 trig v(bd_a0) val='ddv/2'
+ val='ddv/2' rise=3
.meas tran m4 trig v(bd_a0) val='ddv/2'
+ val='ddv/2' rise=4
.meas tran m5 trig v(bd_a0) val='ddv/2'
+ val='ddv/2' rise=5
fall=1
targ v(re_bd)
fall=2
targ v(re_bd)
rise=2
targ v(re_bd)
fall=3
targ v(re_bd)
rise=3
targ v(re_bd)
In this example, when either m1 and m2 are obtained or just m4 is obtained,
the transient analysis ends.
See Also
.MEASURE (Rise, Fall, Delay, and Power Measurements)
368
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION AUTOSTOP (or) .OPTION AUTOST
.MEASURE (FIND and WHEN)
.MEASURE (Continuous Results)
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
.MEASURE (Integral Function)
.MEASURE (Derivative Function)
.MEASURE (Error Function)
.MEASURE PHASENOISE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
369
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_ACTIVE
.OPTION BA_ACTIVE
Specifies the active net file name(s) selective net back-annotation.
Syntax
.OPTION BA_ACTIVE = "FILENAME [;FILENAME2; FILENAME3...]"
Description
Conducts selective back-annotation. The active net file name contains the
selected nets in the format defined by Star-RC or Star-RCXT. If no file is
supplied, all nets (nodes) are selected for annotation. Multiple active net files
can be specified, with each other being delimited by semicolon.
You must use this option with BA_FILE, or it has no effect. To view examples of
active net files used in a format for Star-RC/Star-RCXT, see Selective Net
Back-Annotation in the HSPICE User Guide: Simulation and Analysis.
Examples
.option ba_active = "./hspice/NETLIST/DSPF/active.rcxt"
See Also
.OPTION BA_ACTIVEHIER
.OPTION BA_FILE
Back-Annotation Demo Cases
370
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_ACTIVEHIER
.OPTION BA_ACTIVEHIER
Annotate full hierarchical net names that are specified for BA_ACTIVE files.
Syntax
.OPTION BA_ACTIVEHIER = 0|1
Default 0
Description
Setting this option to 1 annotates the full hierarchical net names that are
specified in BA_ACTIVE files, instead of the name starting from last period (.).
For example, in an active net file, if the net name is xi1.xi2.net_name, by
default, HSPICE truncates this name from the last period and identifies the net
name as 'net_name'. If you set ba_activehier=1, HSPICE use the full net
name.
See Also
.OPTION BA_ACTIVE
Post-Layout Back-Annotation
Back-Annotation Demo Cases
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
371
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_ADDPARAM
.OPTION BA_ADDPARAM
Specifies extra parameters to be scaled by .OPTIONS BA_SCALE/
BA_GEOSHRINK.
Syntax
.OPTION BA_ADDPARAM = "LINEAR: PARAM [PARAM2 …];
+ QUAD: PARAM [PARAM2 …]"
Argument
Description
LINEAR/QUAD
Keywords to indicate how the following parameters to be scaled
for instances in the DPF file, i.e., to be scaled linearly/
quadratically.
PARAM
Parameter to be scaled by .OPTIONS BA_SCALE/
BA_GEOSHRINK. Multiple parameters can be specified, with
each other being delimited by blank space. The parameter
groups (LINEAR/QUAD) are delimited by semicolon.
Description
.OPTION BA_SCALE/BA_GEOSHRINK is usually applied only to common
elements (M/D/R/C/J) and common parameters needed for scaling (L/W/AD/
AS/PD/PS/AREA …). At times, extra, unusual parameters need to be scaled
by BA_SCALE/BA_GEOSHRINK as well, such as the variation of common
parameters from a subckt wrapping a type of element. For example, see a
subckt wrapping a MOSFET with parameters wr/lr, which stands for width/
length of the wrapped MOSFET in the following example.
Examples
.OPTION BA_ADDPARAM
= "LINEAR: WR LR; QUAD: ASR AREAR"
See Also
.OPTION BA_SCALE
.OPTION BA_GEOSHRINK
372
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_COUPLING
.OPTION BA_COUPLING
Controls how to treat cutoff coupling capacitors when invoking selective net
back-annotation.
Syntax
.OPTION BA_COUPLING = 0|1|2
Default 0
Description
Coupling capacitors across two nets are very common in parasitic netlists. For
example, assume one coupling capacitor CC with terminals connected to two
nodes belonging to nets A and B, respectively. When selective net backannotation is launched and net A is active while net B is inactive, then CC is cut
off from the node under net B and the terminal becomes a dangling node.
.OPTION BA COUPLING allows three methods to deal with the cutoff coupling
capacitor, with BA_COUPLING assigned a value listed below:
■
0: Just discards this coupling capacitor (a warning is issued).
■
1: Let the cutoff terminal connect to the node defined by *|GROUND_NET.
■
2: Let the cutoff terminal connect to the unexpanded inactive node (node B
in the example above).
Examples
.OPTION BA_COUPLING = 2
See Also
Post-Layout Back-Annotation
Back-Annotation Demo Cases
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
373
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_DPFPFX
.OPTION BA_DPFPFX
Prepends an extra prefix when searching the ideal netlist for instances
referenced by the parasitic file (DSPF/SPEF/DPF).
Syntax
.OPTION BA_DPFPFX= "string"
Default m_ prefix string
Description
BA_DPFPFX causes HSPICE to prepend an extra prefix when searching the
ideal netlist for instances referenced by the parasitic file (DSPF/SPEF/DPF).
This option serves a different purpose from .OPTION BA_DPFPFX in that
BA_DPFPFX is used to indicate the prefix that has been prepended to instances
in the parasitic file while BA_IDEALPFX is used to specify the extra prefix to be
prepended. This option aids in precisely specifying backward-annotation.
HSPICE automatically checks for a reverse hierarchy in device name. But if the
name is prepended with a prefix string, you need to specify that prefix string
using .OPTION BA_DPFPFX so HSPICE can correctly extract the hierarchical
name.
See Also
.OPTION BA_IDEALPFX
374
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_ERROR
.OPTION BA_ERROR
Mode for handling error on nets.
Syntax
.OPTION BA_Error=0|1|2
Default 1 (LUMPCAP)
Description
Specifies means to handle an error on nets, where:
■
0: EXIT — Terminates the simulation with an error message
■
1: LUMPCAP — Adds only the total lumped net capacitance
■
2: YES — Expands whatever can be expanded
Examples
.OPTION BA_ERROR = 2
See Also
Post-Layout Back-Annotation
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
375
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_FILE
.OPTION BA_FILE
Launches DPF parasitic back-annotation.
Syntax
.OPTION BA_FILE = “FILENAME [;FILENAME2; FILENAME3 …]”
Description
This option enables you to specify the DPF file and invoke DPF backannotation. This option expands usage so that a DSP file does not have to be
embedded in a DSPF file as the “Instance Section.”
FILENAME is the name of the file that contains parasitic information in SPEF or
DSPF format. Multiple parasitic netlists can be specified, with each other being
delimited by semicolon. These parasitic netlists must be independent but
cannot cross-reference each other. The advantage of DPF back-annotation is
that the pre-layout hierarchy is maintained for simulation.
For MOSFET devices, the supported DPF parameters are: L, W, AD, AS, PD,
PS, NRD, NRS, SA, SB, SD, NF, DELVTO, MULU0, RGEOMOD, RDC, RSC,
SCA, SCB, SCC, SA1, SA2, SA3, SA4, SA5, SA6, SA7, SA8, SA9, SA10, SB1,
SB2, SB3, SB4, SB5, SB6, SB7, SB8, SB9, SB10, SW1, SW2, SW3, SW4,
SW5, SW6, SW7, SW8, SW9, SW10.
Use .OPTION BA_ACTIVE with .OPTION BA_FILE to launch selective
parasitic expansion. To view examples of the SPEF and DSPF file structures,
see DSPF and SPEF File Structures in the HSPICE User Guide: Simulation
and Analysis.
Examples
Example 1
Single Parasitic Netlist
.OPTION BA_FILE = "./hspice/NETLIST/DSPF/add4.spf"
Example 2
Multiple Parasitic Netlists
.OPTION BA_FILE = "./ba_file1.spf; ba_file2.spf; ba_file3.spef"
See Also
Full Back-Annotation
Back-Annotation Demo Cases
376
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_FINGERDELIM
.OPTION BA_FINGERDELIM
Explicitly specifies the delimiter character used for finger devices.
Syntax
.OPTION BA_FINGERDELIM=character
Default @
Description
Use this option to specify delimiter characters used on fingered devices.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
377
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_GEOSHRINK
.OPTION BA_GEOSHRINK
Element scaling factor used with .OPTION BA_SCALE.
Syntax
.OPTION BA_GEOSHRINK=X
Default Same as .OPTION GEOSHRINK (or its default value)
Description
In addition to .OPTION BA_SCALE, use this option to further scale geometric
parameters of element instances in the DPF file separately, whose default units
are meters. By default the instances in the DPF file are scaled by .OPTION
GEOSHRINK (and SCALE), no difference with instances in the ideal netlist.
When .OPTION BA_GEOSHRINK is specified, the .OPTION GEOSHRINK is
then disabled for instances in the DPF file and BA_GEOSHRINK is applied to
them separately.
The final instance geometric parameters are then calculated as:
final_dimension = original_dimension * BA_SCALE *
BA_GEOSHRINK
The effective scaling factor is the product of the two parameters; HSPICE uses
ba_scale*ba_geoshrink to scale the parameters/dimensions in the DPF
file.
See Also
.OPTION BA_SCALE
.OPTION SCALE
.OPTION GEOSHRINK
378
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_HIERDELIM
.OPTION BA_HIERDELIM
Specifies the hierarchical separator in the DPF file.
Syntax
.OPTION BA_HIERDELIM=character
Description
If the hierarchical separator used in a DPF file is different from
BA_HIERDELIM, the hierarchical separator must be specified with
BA_HIERDELIM.
Examples
.OPTION BA_HIERDELIM=/
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
379
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_IDEALPFX
.OPTION BA_IDEALPFX
Instructs the simulator to add a second prepended prefix when doing a search
of the ideal netlist.
Syntax
.OPTION BA_IDEALPFX = "m_"
Description
BA_IDEALPFX instructs HSPICE to prepend an extra prefix when searching
the ideal netlist for instances referenced by the parasitic file (DSPF/SPEF/
DPF). Note that a different purpose is served here than when using .OPTION
BA_DPFPFX in that BA_DPFPFX is used to indicate the prefix that has been
prepended to instances in the parasitic file, while BA_IDEALPFX is used to
specify the extra prefix to be prepended.
See Also
.OPTION BA_DPFPFX
380
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_MERGEPORT
.OPTION BA_MERGEPORT
Controls whether to merge net ports into one node.
Syntax
.OPTION BA_MERGEPORT = 0|1
Default 1
Description
Merging net ports into one node may introduce some small inaccuracy. To
separate the net ports, set BA_MERGEPORT = 0.
Examples
.OPTION BA_MERGEPORT = 0
See Also
Post-Layout Back-Annotation
Back-Annotation Demo Cases
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
381
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_NETFMT
.OPTION BA_NETFMT
Specifies the format of Active Net File.
Syntax
.OPTION BA_NETFMT=[1|2]
Default 1
Argument Description
1
Reports active nets in StarRC (*.rcxt) format for the Selective Net
Extraction Flow.
2
Reports active nets in HSIM Back-Annotation (*.hsimba) format for the
Selective Net Back-Annotation Flow.
Description
Enables HSPICE to output active nodes in STAR-RCXT format or HSIMBA
format.
382
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_PRINT
.OPTION BA_PRINT
Controls whether to output nodes and resistors/capacitors introduced by backannotation.
Syntax
.OPTION BA_PRINT = IDEAL|ALL
Default IDEAL
Description
Specify this option to control the output of nodes and resistors/capacitors
added by back-annotation.
After back-annotation many nodes and resistors/capacitors are introduced in
the output files, which can distract from the effective and useful information. By
setting BA_PRINT=IDEAL, the newly-added nodes and resistors/capacitors by
back-annotation are filtered from the *.lis, *.ic# and *.tr#. To switch on the
output of these nodes and RCs, set BA_PRINT=ALL.
Examples
.OPTION BA_PRINT=IDEAL
See Also
Post-Layout Back-Annotation
Back-Annotation Demo Cases
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
383
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_SCALE
.OPTION BA_SCALE
Sets the element scaling factor for instances in the DPF file separately.
Syntax
.OPTION BA_SCALE=X
Default Same as .OPTION SCALE (or its default value)
Description
Use this option to scale geometric parameters of element instances in the DPF
file separately, whose default unit is meters. By default the instances in the DPF
file are scaled by .OPTION SCALE, no difference with instances in the ideal
netlist. When .OPTION BA_SCALE is specified, the .OPTION SCALE is then
disabled for instances in the DPF file and BA_SCALE is applied to them
separately.
You can also use this option with .OPTION BA_GEOSHRINK to scale an
element even more finely. The effective scaling factor is the product of the two
parameters; HSPICE uses ba_scale*ba_geoshrink to scale the
parameters/dimensions in the DPF file.
See Also
.OPTION BA_GEOSHRINK
.OPTION SCALE
.OPTION GEOSHRINK
384
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_TERMINAL
.OPTION BA_TERMINAL
Specifies mapping characters for back annotation terminal name.
Syntax
.OPTION BA_TERMINAL = "TERMINAL= ALIAS [; TERMINAL2= ALIAS2;
+ TERMINAL3=ALIAS3 …]"
Argument
Description
TERMINAL
Terminal name used in the parasitic netlist.
ALIAS
Common terminal name recognized by the simulator, or user-defined/
tool-specific terminal name used in the ideal netlist.
Description
Specifies the terminal name mapping between the parasitic netlist and the
terminal names recognized by the simulator. Multiple TERMINAL=ALIAS pairs
can be specified, with each other being delimited by semicolon. Generally,
terminal names used in the parasitic netlist and ideal netlist are same. These
terminals are widely accepted by various simulators, as listed in the following
table.
Table 1
Default rules for element terminal names
Term. M (MOS)
Index
Q (BJT)
1
C [O] [L] [L] [E] [C] [T] [O] [R] A [N] [O] [D] [E],
D [R] [A] [I] [N]
R,C,D (Resistor, Capacitor,
Diode)
P [L] [U] [S],
P [O] [S] [I] [T] [I] [V] [E]
2
G [A] [T] [E]
B [A] [S] [E]
B,
C [A] [T] [H] [O] [D [E],
M [I] [N] [U] [S],
N [E] [G] [A] [T] [I] [V] [E]
3
S [O] [U] [R] [C] [E] E [M] [I] [T] [T] [E] [R]
4
B [U] [L] [K]
S [U] [B] [S] [T] [R] [A] [T] [E]
S [U] [B] [S] [T] [R] [A] [T] [E] N/A
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
385
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BA_TERMINAL
HPSICE uses the first character and optional subsequent characters listed
above to determine which terminal is referred to.
However, sometimes terminal names referenced in the parasitic netlist are
user-defined/tool-specific and different from above default terminal characters.
Another case is the terminal names employed in the parasitic netlist follow the
default rules, but are different from the ones used in ideal netlist, which are
user-defined/tool-specific. This is especially common for elements of subckt
type. That's what BA_TERMINAL is intended for.
.OPTION BA_TERMINAL is used to set up the terminal name mapping
between the parasitic netlist and ideal netlist. Of the TERMINAL ALIAS pair,
the first entry is the terminal name used in the parasitic netlist, and the second
entry is the corresponding terminal name used in the ideal netlist.
Note:
Consider the following limitation for BA_TERMINAL. All terminal
mapping pairs specified are of global scope, not only applied for
specific elements/blocks, but applicable for all un-found terminal
names. Besides, if multiple mapping pairs have the same first
entry (key), e.g., .OPTION BA_TERMINAL = "UDRN=N1;
UDRN=N2", then the latter pair will hide the previous one and
take effect.
Examples
Example 1
This example maps user-defined terminals (UDRN, UGATE) in the
parasitic netlist to default terminal characters (D, G).
.OPTION BA_TERMINAL="UDRN=D; UGATE=G"
Example 2
This example maps widely accepted terminal characters (D, G, S) in the
parasitic netlist to subckt-defined node list (SUBCKT_N1, SUBCKT_N2,
SUBCKT_N3) in the ideal netlist.
.OPTION BA_TERMINAL="D SUBCKT=N1; G=SUBCKT_N2; S=SUBCKT_N3"
See Also
Post-Layout Back-Annotation
Back-Annotation Demo Cases
386
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BADCHR
.OPTION BADCHR
Generates a warning on finding a nonprintable character in an input file.
Syntax
.OPTION BADCHR=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to generate a warning on finding a nonprintable character in an
input file by setting to 1.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
387
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BDFATOL
.OPTION BDFATOL
Sets the absolute tolerance for the global accuracy control of the Backward
Differentiation Formulae integration method.
Syntax
.OPTION BDFATOL=val
Default
1e-3
Description
Use this option to set the absolute tolerance of the circuit convergence
integration method BDF (a higher order integration algorithm than BackwardEuler, Gear, or Trapezoidal).
The option operates independent of .OPTIONS RUNLVL and ACCURATE
settings with the following exception:
If either .OPTION RUNLVL or ACCURATE follows an .OPTION BDFATOL or
BDFRTOL value, the RUNLVL or ACCURATE setting overrides the tolerance of
the BDF algorithm. If ACCURATE is set with or without RUNLVL, the default for
BDFATOL will always set to 1.e-5.
RUNLVL
BDFATOL
0
1e-4
1
1e-2
2
1e-2
3
1e-3
4
1e-4
5
1e-4
6
1e-5
The option appears in the .lis file.
Examples
.OPTION METHOD=BDF
+.OPTIONS BDFATOL=1e-4 BDFRTOL=1e-4
388
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BDFATOL
See Also
.OPTION METHOD
.OPTION BDFRTOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
389
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BDFRTOL
.OPTION BDFRTOL
Sets the relative tolerance for the global accuracy control of the Backward
Differentiation Formulae integration method.
Syntax
.OPTION BDFRTOL=val
Default
1e-3
Description
Use this option to set the relative tolerance of the circuit convergence
integration method BDF (a higher order integration algorithm than BackwardEuler, Gear, or Trapezoidal).
The option operates independent of .OPTIONS RUNLVL and ACCURATE
settings with the following exception:
If .OPTION RUNLVL or ACCURATE follows an .OPTION BDFATOL or
BDFRTOL value, the RUNLVL or ACCURATE setting overrides the tolerance of
the BDF algorithm. If ACCURATE is set with or without RUNLVL, the default for
BDFRTOL will always reset to 1.e-5.
RUNLVL
BDFRTOL
0
1e-4
1
1e-2
2
1e-2
3
1e-3
4
1e-4
5
1e-4
6
1e-5
The value of the option appears in the .lis file.
Examples
.OPTION METHOD=BDF
+.OPTIONS BDFRTOL=1e-4 BDFATOL=1e-4
390
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BDFRTOL
See Also
.OPTION METHOD
.OPTION BDFATOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
391
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BEEP
.OPTION BEEP
Enables or disables audible alert tone when simulation returns a message.
Syntax
.OPTION BEEP=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to enable or disable the audible alert tone when simulation
returns a message.
392
■
BEEP=1 Turns on an audible tone when simulation returns a message (such
as HSPICE job completed).
■
BEEP=0 Turns off the audible tone.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BIASFILE
.OPTION BIASFILE
Sends .BIASCHK command results to a specified file.
Syntax
.OPTION BIASFILE=file_name
Default
*.lis
Description
Use this option to output the results of all .BIASCHK commands to a file that
you specify. If you do not set this option, HSPICE outputs the .BIASCHK
results to the *.lis file.
Examples
.OPTION BIASFILE=’biaschk/mos.bias’
See Also
.BIASCHK
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
393
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BIASINTERVAL
.OPTION BIASINTERVAL
Controls the level of information output during transient analysis.
Syntax
.OPTION BIASINTERVAL=[0|1|2|3]
Description
Use this option with the .BIASCHKinterval argument to control the level of
information output during transient analysis.
■
BIASINTERVAL=0: Ignores the interval argument.
■
BIASINTERVAL=1: Output the total number of suppressed violation regions
for those elements being monitored. Violation warning messages that are
generated in these suppressed regions are removed from the output.
■
BIASINTERVAL=2: Output detailed information regarding suppressed
violation regions. This includes element information, start time, stop time,
and peak values. Also, violation warning messages that are generated in
these suppressed regions are removed from the output.
■
BIASINTERVAL=3: Output detailed information about all violation regions.
Also, violation warning messages that are generated in these regions are
removed from the output.
Examples
.OPTION BIASINTERVAL=1
See Also
.BIASCHK
394
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BIASNODE
.OPTION BIASNODE
Specifies whether to use node names or port names in element commands.
Syntax
.OPTION BIASNODE=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to specify whether to use node names or port names in element
commands in .BIASCHK warning messages.
■
BIASNODE=1: use node names instead of port names
■
BIASNODE=0: use port names (for example, ng of MOS element)
Examples
.OPTION BIASNODE=1
See Also
.BIASCHK
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
395
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BIASPARALLEL
.OPTION BIASPARALLEL
Controls whether .BIASCHK sweeps the parallel elements being monitored.
Syntax
.OPTION BIASPARALLEL=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option with the .BIASCHKmname argument to control whether
.BIASCHK sweeps the parallel elements being monitored.
■
BIASPARALLEL=1: sweep parallel elements. If node voltage is also being
monitored, only the first element is used to generate warning messages.
■
BIASPARALLEL=0: do not sweep parallel elements.
Examples
.OPTION BIASPARALLEL=1
See Also
.BIASCHK
396
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BIAWARN
.OPTION BIAWARN
Controls whether HSPICE outputs warning messages when local max bias
voltage exceeds limit during transient analysis.
Syntax
.OPTION BIAWARN=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to control whether HSPICE outputs warning messages when a
local max bias voltage exceeds the limit during transient analysis.
■
BIAWARN=1: Output warning messages. When transient analysis is
completed, the results are output as filtered by noise.
■
BIAWARN=0: Do not output a warning message. When the transient
analysis is completed, output the results.
Examples
.OPTION BIAWARN=1
See Also
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
397
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BINPRNT
.OPTION BINPRNT
Outputs the binning parameters of the CMI MOSFET model.
Syntax
.OPTION BINPRNT=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to output the binning parameters of the CMI MOSFET model.
Currently available only for Level 57.
398
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BPNMATCHTOL
.OPTION BPNMATCHTOL
Determines the minimum required match between the NLP and PAC phase
noise algorithms in HSPICE RF.
Syntax
.OPTION BPNMATCHTOL=val
Default 0.5dB
Description
Use this option to determines the minimum required match between the NLP
and PAC phase noise algorithms. An acceptable range is 0.05dB to 5dB.
See Also
.OPTION PHASENOISEKRYLOVDIM
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER
.OPTION PHASENOISETOL
.OPTION PHNOISELORENTZ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
399
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BRIEF
.OPTION BRIEF
Stops echoing (printback) of data file to stdout until HSPICE reaches
an .OPTION BRIEF=0 or .END command.
Syntax
.OPTION BRIEF=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to terminate echoing (printback) of the data file to stdout until
HSPICE finds an .OPTION BRIEF=0 or the .END command. It also resets the
LIST, NODE and OPTS options, and sets NOMOD. BRIEF=0 enables printback.
The NXX option is the same as BRIEF. BRIEF=1 disables
printback. .OPTION BRIEF=1 and .OPTION BRIEF=0 act similar to the
commands .PROTECT and .UNPROTECT, respectively.
For information on how BRIEF impacts other options, see Appendix B, How
Options Affect other Options.
Examples
This example shows how, if you include in your netlist .option brief=0, the
printback of the library file would be prevented but the list option would work.
.option brief
.lib 'mymodels.lib' tt
.option brief=0
See Also
.END
.OPTION LIST
.OPTION NODE
.OPTION NXX
.OPTION OPTS
.PROTECT or .PROT
.UNPROTECT or .UNPROT
400
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BSIM4PDS
.OPTION BSIM4PDS
Flag to control the BSIM4 Pseff (effective source perimeter) and Pdeff (effective
drain perimeter) model equation calculation.
Syntax
.OPTION BSIM4PDS=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Setting BSIM4PDS=1 enhances the pseff and pdeff calculation, so that when the
calculated pseff and pdeff is negative, HSPICE uses the PAeffGeo function to
recalculate it. (This option solves the issue of negative pseff and pdeff causing
potential non-convergence issues.) When BSIM4PDS=0, HSPICE strictly
follows the UCB code, and results in no recalculation if negative pseff or pdeff
occurs.
Note:
This option is only available for BSIM4 (Level 54).
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
401
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BYPASS
.OPTION BYPASS
Bypasses model evaluations if the terminal voltages stay constant.
Syntax
.OPTION BYPASS=[0|1|2]
Default
1 for MESFETs, JFETs, or BJTs; 2 for MOSFETs and diodes
Description
Use this option to bypass model evaluations if the terminal voltages do not
change. Values can be 0 (off), 1 (on), or 2 (advanced algorithm, applies to
BSIM3v3, BSIM4, BSIM3SOI (LEVEL=57), BSIM4SOI (LEVEL 70), HVMOS
(LEVEL 66), and PSP (LEVEL=69) MOSFETs in special cases).
To speed up simulation, BYPASS=1 does not update the status of latent
devices. BYPASS=2 uses linear prediction to update the devices and balance
speed and accuracy.
(Assuming BYPASS is not explicitly set otherwise): When the BYPASS option is
not given in the netlist, its value is determined by the value of RUNLVL and
ACCURATE. When RUNLVL=0 then BYPASS=1; when RUNLVL=0 +
ACCURATE=1 then BYPASS=0; when RUNLVL=1 through 6, then BYPASS=2.
See Also
.OPTION ACCURATE
.OPTION RUNLVL
402
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION BYTOL
.OPTION BYTOL
Sets a voltage tolerance at which a MOSFET, MESFET, JFET, BJT, or diode
becomes latent.
Syntax
.OPTION BYTOL=x
Default
100.00u
Description
Use this option to specify a voltage tolerance at which a MOSFET, MESFET,
JFET, BJT, or diode becomes latent. HSPICE does not update status of latent
devices. The default=MBYPASS x VNTOL.
See Also
.OPTION MBYPASS
.OPTION VNTOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
403
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CAPTAB
.OPTION CAPTAB
Adds up all the capacitances attached to a node and prints a table of singleplate node capacitances.
Syntax
.OPTION CAPTAB=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to print a compiled table of single-plate node capacitances for
diodes, BJTs, MOSFETs, JFETs, and passive capacitors at each operating
point.
Note:
404
When .OPTION CAPTAB is used to estimate the equivalent
capacitance of the circuit nodes, HSPICE can give a zero
capacitance values for some nodes when a resistance is
connected to that node. The reason for getting 0 is that the
capacitance is a dynamic, frequency-dependent capacitance
and not a static capacitance. You need to run an AC analysis to
see a non-zero node capacitance.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CFLFLAG
.OPTION CFLFLAG
Activates the Compiled Function Library (CFL) feature in HSPICE.
Syntax
.OPTION CFLFLAG=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to turn on the CFL capability and pass arguments
(mathematical or user-defined functions written in C that can be dynamically
linked to HSPICE during run time). See the Features section of the HSPICE
User GUIDE: Simulation and Analysis for more information.
Examples
In the following example, mysqrt(x) and func(arg1, arg2) are a coded
as a CFL function. The functions mysqrt and func are called in the netlist as
follows:
.option CFLflag
.param area = 4u*u
.param p1 = mysqrt(area)
.param p2 = mysqrt(area/2)
.param p3 = func(p1, p2)
See Also
.CFL_PROTOTYPE
.PARAM (or) .PARAMETER (or) .PARAMETERS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
405
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CHGTOL
.OPTION CHGTOL
Sets a charge error tolerance.
Syntax
.OPTION CHGTOL=x
Default
1.00f
Description
Use this option to set a charge error tolerance if you set LVLTIM=2. Use
CHGTOL with RELQ to set the absolute and relative charge tolerance for all
HSPICE capacitances. The default is 1e-15 (coulomb). Min value: 1e-20; Max
value: 10.
See Also
.OPTION CHGTOL
.OPTION LVLTIM
.OPTION RELQ
406
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CMIMCFLAG
.OPTION CMIMCFLAG
Restricted: for specified users only. Enables model memory allocation for each
element.
Syntax
.OPTION CMIMCFLAG=0|1
Default 0
Description
For restricted use: Setting this option to 1, changes the method for storing
instance-specific local variation information. With use of this flag, during the
instance reset process model memory is allocated for each element. Each
instance will have its own model structure to store the local variation
information.
Note:
Users employing conventional public domain models where
many model parameters exist should not use this option to avoid
memory issues.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
407
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CMIFLAG
.OPTION CMIFLAG
Loads and links the dynamically linked Common Model Interface (CMI) library.
Syntax
.OPTION CMIFLAG=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to load and link the compiled CMI object .so file to HSPICE/
HSPICE RF during simulation runs. If this option parameter is set with no value
or to 1, then the CMI .so file is loaded as a dynamically-linked object file. If this
option parameter does not exist (deemed as default) in the netlist, or is
explicitly set to 0, no loading or linking takes place.
If CMIFLAG is set, model parameter CMIMODEL can be used to enable “hybrid”
model usage, i.e., you can determine if a built-in model or model from custom
CMI library is to be used in the simulation.
CMIMODEL=0|1|2|undefined
Model parameter CMIMODEL values are as follows:
■
0: HSPICE searches for the model from built-in models. If not found, an error
message is issued and HSPICE aborts.
■
1: HSPICE searches for the model from the Custom CMI. If not found, a
warning message is issued and HSPICE then searches for the model from
built-in models.
■
2: Invokes the CMI2 mode.
■
undefined: HSPICE proceeds as if CMIMODEL=1.
If .OPTION CMIFLAG is not set, model parameter CMIMODEL is ignored.
See Also
.OPTION CUSTCMI
408
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CMIPATH
.OPTION CMIPATH
Enables automatic selection of correct Custom CMI .so library platform. For
information on the HSPICE CMI, contact your Synopsys technical support
team.
Syntax
.OPTION CMIPATH='LIB_DIRECTORY'
Description
This option allows you to automatically select the correct custom CMI .so
library platform, even though you might not have the right information about the
platform HSPICE is running on. This functionality eliminates the need to
manually search for the correct platform and allows for efficient CMI .so library
distribution and customer applications. The solution to this issue keeps the
environment variable hspice_lib_models backward compatible in its usage
model, but users can add the control option .OPTION
CMIPATH='LIB_DIRECTORY' to the model file.
For the UNIX OS, HSPICE provides two scripts, hspice and hspice64 to
invoke the right HSPICE executable for the platform on which HSPICE is being
invoked to run. These scripts are enhanced to recognize the correct machine
and platform for automatic CMI .so library selection. For the Windows OS, no
HSPICE script is required, since all Windows platforms share the same single
CMI .so library:LIB_DIRECTORY/WIN for all Windows platforms.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
409
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CMIUSRFLAG
.OPTION CMIUSRFLAG
Flag to control.OPTION SCALE parsing into the External Common Model
Interface (CMI).
Syntax
.OPTION CMIUSRFLAG=0|1|2|3
Default
0
Description
Controls the CMI element instance parameter value (unit) scaling. This option
is only available for custom CMI MOS Level 101. It permits users and/or
foundry model development teams to choose desired scaling for the instance
parameters of the MOSFET devices that call a foundry’s CMI model libraries.
The CMIUSRFLAG values are as follows:
■
0: Turns off other functions of the CMIUSRFLAG option.
■
1: Passes scale*geoshrink value to custom CMI through artificial
instance parameter “scale”. If set with no value or to 1, the products of option
parameters SCALE and GEOSHRINK are passed and made available to
scale the CMI model instance parameter values.
■
2: Turns on dynamic model bin selection for custom CMI and turns off other
functions.
■
3 HSPICE will pass options SHRINK, SCALE and M into Custom CMI (both
MOSFET model with BSIM4-like topology and DIODE model), using string
names "optshrink", "optscale", and "mult", respectively. In
addition, final constant capacitance value (for capacitors) will be scaled by
.OPTION SHRINK.
If the CMIUSRFLAG option parameter does not exist in the netlist (default), or is
explicitly set to 0, then the option parameters SCALE and GEOSHRINK are not
accessible in the CMI; and the element instance parameter scaling is not
activated for the foundry CMI models and libraries.
Examples
In this example, the value scale*geoshrink=0.9e-6 is parsed to the
external CMI.
.option cmiflag=1
.option scale=1e-6 geoshrink=0.9 cmiusrflag=1
...
.model nch nmos level=101 ...
410
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CMIUSRFLAG
See Also
.OPTION SCALE
.OPTION GEOSHRINK
.OPTION SHRINK
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
411
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CONVERGE
.OPTION CONVERGE
Invokes various methods for solving nonconvergence problems.
Syntax
.OPTION CONVERGE=[-1|0|1|2|3|4|5|100]
Description
Use this option to run different methods for solving nonconvergence issues.
This option is part of the autoconverge flow.
Note:
In HSPICE RF, this option is ignored because it is replaced by
automated algorithms.
■
CONVERGE=-1: Use with DCON=-1 to disable autoconvergence.
■
CONVERGE=0: Autoconvergence.
■
CONVERGE=1: Use the Damped Pseudo Transient algorithm. If simulation
does not converge within the set CPU time (in the CPTIME control option),
then simulation halts.
■
CONVERGE=2: Use a combination of DCSTEP and GMINDC ramping. Not
used in the autoconvergence flow.
■
CONVERGE=3: Invoke the source-stepping method. Not used in the
autoconvergence flow.
■
CONVERGE=4: Use the gmath ramping method.
■
CONVERGE=5: Use the gshunt ramping method. Even you did not set it in
an .OPTION command, the CONVERGE option activates if a matrix floatingpoint overflows or if HSPICE reports a “timestep too small” error. The default
is 0. If a matrix floating-point overflows, then CONVERGE=1.
■
CONVERGE=100 Adaptive option control for autoconvergence; this value
requires less dependence on convergence option settings, such as DV,
ITL1, GRAMP, SYMB, and DCON.
See Also
.OPTION DCON
.OPTION GMINDC
.OPTION DV
.OPTION GRAMP
.OPTION ITL1
.OPTION SYMB
412
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CPTIME
.OPTION CPTIME
Sets the maximum CPU time allotted for a simulation.
Syntax
.OPTION CPTIME=x
Default
10.00x
Description
Use this option to set the maximum CPU time, in seconds, allotted for this
simulation job. When the time allowed for the job exceeds CPTIME, HSPICE
prints or plots the results up to that point and concludes the job. Use this option
if you are uncertain how long the simulation takes, especially when you debug
new data files. The default is 1e7 (400 days).
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
413
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CSCAL
.OPTION CSCAL
Sets the capacitance scale for Pole/Zero analysis.
Syntax
.OPTION CSCAL=x
Default
1.0e+12
Description
Use this option to set the capacitance scale for Pole/Zero analysis. HSPICE
multiplies capacitances by CSCAL.
See Also
.OPTION FMAX
.OPTION GSCAL
.OPTION ITLPZ
.OPTION LSCAL
.OPTION PZABS
414
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CSDF
.OPTION CSDF
Selects the Common Simulation Data Format (Viewlogic-compatible graph
data file format).
Syntax
.OPTION CSDF=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to specify whether HSPICE/ HSPICE RF outputs CSDF data
when you run a HSPICE simulation.
■
If CSDF=0, CSDF output is disabled.If CSDF=1, HSPICE produces CSDF
output.
See Also
.OPTION POST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
415
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CSHDC
.OPTION CSHDC
Adds capacitance from each node to ground; used only with the CONVERGE
option.
Syntax
.OPTION CSHDC=x
Description
Use this option to add capacitance from each node to ground. This is the same
option as CSHUNT; use CSHDC only with the CONVERGE option. When
defined, .OPTION CSHDC is the same as .OPTION CSHUNT, except that
CSHDC becomes invalid after DC OP analysis, while CSHUNT stays in both
DC OP and transient analysis.
See Also
.OPTION CONVERGE
.OPTION CSHUNT
416
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CSHUNT
.OPTION CSHUNT
Adds capacitance from each node to ground.
Syntax
.OPTION CSHUNT=x
Default
0
Description
Use this option to add capacitance from each node to ground. Add a small
CSHUNT to each node to solve internal “timestep too small” timestep problems
caused by high frequency oscillations or numerical noise. When defined,
.OPTION CSHUNT is the same as .OPTION CSHDC, except that CSHDC
becomes invalid after DC OP analysis, while CSHUNT stays in both DC OP and
transient analysis.
Examples
.option
.option
.option
.option
.option
gshunt=1e-13
gshunt=1e-12
gshunt=1e-11
gshunt=1e-10
gshunt=1e-9
cshunt=1e-17
cshunt=1e-16
cshunt=5e-15
cshunt=1e-15
cshunt=1e-14
See Also
.OPTION CSHDC
.OPTION GSHUNT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
417
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CUSTCMI
.OPTION CUSTCMI
Turns on gate direct tunneling current modeling and additional instance
parameter support.
Syntax
.OPTION CUSTCMI= 0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to turn on gate direct tunneling current modeling and instance
parameter support. Set .OPTION CUSTCMI=1 jointly with .OPTION CMIFLAG
to turn on gate direct tunneling current modeling and instance parameters.
.OPTION CUSTCMI=0 to turns off the feature.
The existing HSPICE BSIM4-like instance parameters include: geomod,
acnqsmod, delk1, delnfct, deltox, min, mulu0, nf, rbdb, rbodymod, rbpb, rbpd,
rbps, rbsb, rgatemod, sa, sa1, sa10,sa2, sa3, sa4, sa5, sa6, sa7,sa8, sa9, sb,
sb1, sb10, sb2,sb3, sb4, sb5, sb6, sb7, sb8,sb9, sd, stimod, sw1, sw10, sw2,
sw3, sw4, sw5, sw6, sw7, sw8, sw9, and trnqsmod.
.OPTION CUSTCMI=1 also supports the six integer instance model flags:
insflg1, insflg2, insflg3, insflg4, insflg5, and insflg6 and the
ten double precision instance parameters supported for customer CMI:
insprm1, insprm2, insprm3, insprm4,...,insprm10.
See Also
.OPTION CMIFLAG
418
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION CVTOL
.OPTION CVTOL
Changes the number of numerical integration steps when calculating the gate
capacitor charge for a MOSFET.
Syntax
.OPTION CVTOL=x
Description
Use this option to change the number of numerical integration steps when
calculating the gate capacitor charge for a MOSFET by using CAPOP=3. See
the discussion of CAPOP=3 in the “Overview of MOSFET Models” chapter of
the HSPICE Reference Manual: MOSFET Models for explicit equations and
discussion.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
419
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION D_IBIS
.OPTION D_IBIS
Specifies the directory containing the IBIS files.
Syntax
.OPTION D_IBIS=’ibis_files_directory’
Description
Use this option to specify the directory containing the IBIS files. If you specify
several directories, the simulation looks for IBIS files in the local directory (the
directory from which you run the simulation). It then checks the directories
specified through .OPTIOND_IBIS in the order that .OPTION cards appear in
the netlist. You can use the D_IBIS option to specify up to 40 directories.
Examples
.OPTION d_ibis='/home/user/ibis/models'
420
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCAP
.OPTION DCAP
Specifies equations used to calculate depletion capacitance for Level 1 and 3
diodes and BJTs.
Syntax
.OPTION DCAP
Description
Use this option to specify equations for HSPICE to use when calculating
depletion capacitance for Level 1 and 3 diodes and BJTs. The HSPICE
Reference Manual: Elements and Device Models describes these equations in
the section Using Diode Capacitance Equations.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
421
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCCAP
.OPTION DCCAP
Generates C-V plots.
Syntax
.OPTION DCCAP=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to generate C-V plots. Prints capacitance values of a circuit
(both model and element) during a DC analysis. You can use a DC sweep of
the capacitor to generate C-V plots. If not set, MOS device or voltage-variable
capacitance values are not evaluated and the printed value is zero. When doing
C-V curves for devices, make sure you set .OPTION DCCAP so that the
capacitance values can be output. Depending on the MOS model level you are
using, make sure that you use the appropriate model templates for the models.
See Also
.DC
MOSFET Device Examples, for paths to demo files gatecap.sp and
mosivcv.sp.
422
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCFOR
.OPTION DCFOR
Sets the number of iterations to calculate after a circuit converges in the steady
state.
Syntax
.OPTION DCFOR=x
Default
0
Description
Use this option to set the number of iterations to calculate after a circuit
converges in the steady state. The number of iterations after convergence is
usually zero, so DCFOR adds iterations (and computation time) to the DC circuit
solution. DCFOR ensures that a circuit actually, not falsely, converges.
Use this option with .OPTIONDCHOLD and the .NODESET command to
enhance DC convergence.
See Also
.DC
.NODESET
.OPTION DCHOLD
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
423
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCHOLD
.OPTION DCHOLD
Specifies how many iterations to hold a node at the .NODESET voltage values.
Syntax
.OPTION DCHOLD=n
Default
1
Description
Use this option to specify how many iterations to hold a node at the .NODESET
voltage values.
Note:
In HSPICE RF, this option is ignored; it is replaced by automated
algorithms.
Use DCFOR and DCHOLD together to initialize DC analysis.DCFOR and DCHOLD
enhance the convergence properties of a DC simulation. DCFOR and DCHOLD
work with the .NODESET command. The effects of DCHOLD on convergence
differ, according to the DCHOLD value and the number of iterations before DC
convergence.
If a circuit converges in the steady state in fewer than DCHOLD iterations, the
DC solution includes the values set in .NODESET.
If a circuit requires more than DCHOLD iterations to converge, HSPICE ignores
the values set in the .NODESET command, and calculates the DC solution by
setting the .NODESET fixed-source voltages as open circuited.
See Also
.DC
.NODESET
.OPTION DCFOR
424
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCIC
.OPTION DCIC
Specifies whether to use or ignore .IC commands in the netlist.
Syntax
.OPTION DCIC=0|1
Description
Use this option to specify whether to use or ignore .IC commands in the
netlist.
■
DCIC=1 (default): Each point in a DC sweep analysis acts like an operating
point and all .IC commands in the netlist are used.
■
DCIC=0: .IC commands in the netlist are ignored for DC sweep analysis.
See Also
.IC
.DC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
425
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCON
.OPTION DCON
Aids in the auto-convergence routines; can also disable autoconverge routines
when set to =-1.
Syntax
.OPTION DCON=x
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
This option aids in the autoconvergence routines.
When DCON equals
■
-1: Disables convergence routines, Steps 2 and 3 of the HSPICE
autoconverge process (when DCON=-1 and .OPTION CONVERGE=-1).
■
0: Enables autoconvergence routines as designed
■
1: If a circuit cannot converge using Newton-Raphson, HSPICE
automatically sets DCON=1 and calculates the following:
V max
DV = max ⎛ 0.1, -----------⎞ , if DV =1000
⎝
50 ⎠
I max
GRAMP = max ⎛ 6, log 10 ⎛ -------------------------⎞ ⎞
⎝
⎝ GMINDC⎠ ⎠
■
ITL1 = ITL1 + 20 ⋅ GRAMP
2: If the circuit still cannot converge, HSPICE sets DCON=2, which sets
DV=1e6.
See Also
.OPTION CONVERGE
.OPTION DV
Autoconverge Process
426
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCSTEP
.OPTION DCSTEP
Converts DC model and element capacitors to a conductance.
Syntax
.OPTION DCSTEP=n
Default
0 (seconds)
Description
Use this option to convert DC model and element capacitors to a conductance
to enhance DC convergence properties. HSPICE divides the value of the
element capacitors by DCSTEP to model DC conductance.
See Also
.DC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
427
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DCTRAN
.OPTION DCTRAN
Invokes different methods to solve nonconvergence problems.
Syntax
.OPTION DCTRAN=x
Description
Use this option to run different methods to solve nonconvergence problems.
DCTRAN is an alias for CONVERGE.
See Also
.OPTION CONVERGE
428
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFAD
.OPTION DEFAD
Sets the default MOSFET drain diode area.
Syntax
.OPTION DEFAD=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to set the default MOSFET drain diode area.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
429
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFAS
.OPTION DEFAS
Sets the default MOSFET source diode area.
Syntax
.OPTION DEFAS=x
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to set the default MOSFET source diode area.
430
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFL
.OPTION DEFL
Sets the default MOSFET channel length.
Syntax
.OPTION DEFL=x
Default
100.00u
Description
Use this option to set the default MOSFET channel length.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
431
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFNRD
.OPTION DEFNRD
Sets the default number of squares for the drain resistor on a MOSFET.
Syntax
.OPTION DEFNRD=n
Default
0
Description
Use this option to set the default number of squares for the drain resistor on a
MOSFET.
432
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFNRS
.OPTION DEFNRS
Sets the default number of squares for the source resistor on a MOSFET.
Syntax
.OPTION DEFNRS= n
Default
0
Description
Use this option to set the default number of squares for the source resistor on a
MOSFET.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
433
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFPD
.OPTION DEFPD
Sets the default MOSFET drain diode perimeter.
Syntax
.OPTION DEFPD=n
Default
0
Description
Use this option to set the default MOSFET drain diode perimeter.
434
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFPS
.OPTION DEFPS
Sets the default MOSFET source diode perimeter.
Syntax
.OPTION DEFPS=x
Default
0
Description
Use this option to set the default MOSFET source diode perimeter.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
435
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFSA
.OPTION DEFSA
Sets the default BSIM4 MOSFET SA parameter in HSPICE.
Syntax
.OPTION DEFSA=x
Default
0.0
Description
Use this option to set the default distance between the S/D diffusion edge to the
poly gate edge from one side in the BSIM STI/LOD model.
436
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFSB
.OPTION DEFSB
Sets the default BSIM4 MOSFET SB parameter.
Syntax
.OPTION DEFSB=x
Default
0.0
Description
Use this option to set the default distance between the S/D diffusion edge to the
poly gate edge from side opposite the SA side in the BSIM STI/LOD model.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
437
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFSD
.OPTION DEFSD
Sets default for BSIM4 MOSFET SD parameter.
Syntax
.OPTION DEFSD=x
Default
0.0
Description
Use this option to set the default for the distance between neighboring fingers
(SD parameter) in a BSIM STI/LOD model.
438
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEFW
.OPTION DEFW
Sets the default MOSFET channel width.
Syntax
.OPTION DEFW=x
Default
100.00u
Description
Use this option to set the default MOSFET channel width. The default is 1e-4m.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
439
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEGF
.OPTION DEGF
Sets the device’s failure criteria for lifetime computation when using the
MOSRA API if no values are set for .OPTIONS DEGFN or DEGFP.
Syntax
.OPTION DEGF=val
Description
This option is used in conjunction with .OPTION MOSRALIFE. For NMOS,
DEGFN is used. If DEGFN is not defined, DEGF is used instead.
For PMOS, DEGFP is used. If DEGFP is not defined, DEGF is used instead. This
option sets the device’s degradation value at lifetime. The options apply to all
MOSFETs. The lifetime values are printed in the RADEG file.
See Also
.OPTION DEGFN
.OPTION DEGFP
.OPTION MOSRALIFE
440
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEGFN
.OPTION DEGFN
Sets the NMOS's failure criteria for lifetime computation when using the
MOSRA API.
Syntax
.option DEGFN=val
Description
This option is used in conjunction with .OPTION MOSRALIFE. This option sets
the PMOS's degradation value at lifetime. If the option is not specified or the
keyword can not be identified by the MRAlifetimeDeg function, HSPICE
substitutes .OPTION DEGF for lifetime computation. The options apply to all
MOSFETs. The lifetime values are printed in the RADEG file.
See Also
.OPTION DEGF
.OPTION DEGFP
.OPTION MOSRALIFE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
441
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DEGFP
.OPTION DEGFP
Sets the PMOS's failure criteria for lifetime computation when using the
MOSRA API.
Syntax
.option DEGFP= val
Description
This option is used in conjunction with .OPTION MOSRALIFE. This option sets
the PMOS's degradation value at lifetime. If the option is not specified or the
keyword can not be identified by the MRAlifetimeDeg function, HSPICE
substitutes .OPTION DEGF for lifetime computation. The options apply to all
MOSFETs. The lifetime values are printed in the RADEG file.
See Also
.OPTION DEGF
.OPTION DEGFN
.OPTION MOSRALIFE
442
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DELMAX
.OPTION DELMAX
Sets the maximum allowable step size of the timesteps taken during transient
analysis in HSPICE/HSPICE RF.
Syntax
.OPTION DELMAX=x
Default
(Computed automatically)
Description
Use this option to set the maximum allowable step size of the internal timestep.
The maximum internal timestep taken by HSPICE during transient analysis is
referred to as Δt max . Its value is normally computed automatically based on
several timestep control settings. If you wish to override the automatically
computed value, and force the maximum step size to be a specific value, you
can do so with .OPTION DELMAX, or by specifying a delmax value with the
.TRAN command. If not specified, HSPICE automatically computes a DELMAX
“auto” value, based on timestep control factors such as FS and RMAX.
The initial calculated DELMAX “auto” value, shown in the output listing, is
generally not the value used for simulation. The calculated DELMAX value is
automatically adjusted by the timestep control methods, DVDT, RUNLVL and
LVLTIM.
If DELMAX is defined in an .OPTION command, its priority is higher than the
value given with a .TRAN command and it overrides the DELMAX “auto” value
calculations. Min value: -1e10; Max value 1e10.
See Also
.TRAN
.OPTION DVDT
.OPTION RUNLVL
.OPTION LVLTIM
.OPTION FS
.OPTION RMAX
Appendix B, How Options Affect other Options
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
443
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DI
.OPTION DI
Sets the maximum iteration to iteration current change in HSPICE.
Syntax
.OPTION DI=n
Default
100.00
Description
Use this option to set the maximum iteration to iteration current change through
voltage-defined branches (voltage sources and inductors). Use this option only
if the value of the ABSH control option is greater than 0.
See Also
.OPTION ABSH
444
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DIAGNOSTIC (or) .OPTION DIAGNO
.OPTION DIAGNOSTIC (or) .OPTION DIAGNO
Logs the occurrence of negative model conductances.
Syntax
.OPTION DIAGNOSTIC
Description
Use this option to log the occurrence of negative model conductances.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
445
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DLENCSDF
.OPTION DLENCSDF
Specifies how many digits to include in scientific notation (exponents) or to the
right of the decimal point when using Common Simulation Data Format.
Syntax
.OPTION DLENCSDF=x
Default
5
Description
If you use the Common Simulation Data Format (Viewlogic graph data file
format) as the output format, this digit length option specifies how many digits
to include in scientific notation (exponents) or to the right of the decimal point.
Valid values are any integer from 1 to 10.
If you assign a floating decimal point or if you specify less than 1 or more than
10 digits, HSPICE uses the default. For example, it places 5 digits to the right of
a decimal point.
446
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DV
.OPTION DV
Specifies maximum iteration to iteration voltage change for all circuit nodes in
both DC and transient analyses.
Syntax
.OPTION DV=x
Default
1.00k
Description
Use this option to specify maximum iteration to iteration voltage change for all
circuit nodes in both DC and transient analysis. High-gain bipolar amplifiers can
require values of 0.5 to 5.0 to achieve a stable DC operating point. Large
CMOS digital circuits frequently require about 1 V. The default is 1000 (or 1e6 if
DCON=2).
See Also
.DC
.OPTION DCON
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
447
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DVDT
.OPTION DVDT
Adjusts the timestep based on rates of change for node voltage.
Syntax
.OPTION DVDT=0|1|2|3|4
Default 4 (regardless of runlvl setting)
Description
Use this option to adjust the timestep based on rates of change for node
voltage.
■
0: Original algorithm
■
1: Fast
■
2: Accurate
■
3, 4: Balance speed and accuracy
■
The ACCURATE option also increases the accuracy of the results.
For additional information, see “DVDT Dynamic Timestep” in the HSPICE User
Guide: Simulation and Analysis.
For information on how DVDT values impact other options, see Appendix B,
How Options Affect other Options.
See Also
.OPTION ACCURATE
.OPTION DELMAX
448
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DVTR
.OPTION DVTR
Limits the voltage in transient analysis.
Syntax
.OPTION DVTR=x
Default
1.00k
Description
Use this option to limit the voltage in transient analysis. The default is 1000.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
449
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION DYNACC
.OPTION DYNACC
(Optimization) Dynamic accuracy tolerance setting to accelerate bisection
simulation.
Syntax
.OPTION DYNACC = 0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
When DYNACC=1, if HSPICE is in accuracy mode, it uses reduced accuracy
simulations to narrow the bisection window, then switches to the original
accuracy algorithm to refine the solution. This method reduces simulation time
by doing the majority of simulations at lower accuracy, which run faster by
taking fewer time steps.If DYNACC is set using the .OPTION command, the
setting of DYNACC in .model card is overridden.
See Also
.MODEL
450
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION EM_RECOVERY
.OPTION EM_RECOVERY
Provides a coefficient value for measuring “recovered” average current such as
electromigration for bipolar currents.
Syntax
.OPTION EM_RECOVERY=value
Default
1
Description
This option is used in a transient analysis with the .MEAS keyword em_avg
(electromigration average) using the From-To function. .OPTION
EM_RECOVERY assists in measuring “recovered” average current from an
electromigration perspective. The option can have a coefficient value between
0.0 and 1.0. Recovered average current is especially meaningful for bipolar
currents (for example output of the inverter), as the mathematical average for
such a waveform is zero.
Examples
.option em_recovery=0.9
See Also
.MEASURE (AVG, EM_AVG, INTEG, MIN, MAX, PP, and RMS)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
451
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION EPSMIN
.OPTION EPSMIN
Specifies the smallest number a computer can add or subtract.
Syntax
.OPTION EPSMIN=x
Description
Use this option to specify the smallest number that a computer can add or
subtract, a constant value. This options helps avoid zero denominator issues.
452
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION EXPLI
.OPTION EXPLI
Enables the current-explosion model parameter.
Syntax
.OPTION EXPLI=x
Default
0 (amp/area effective)
Description
Use this option to enable the current-explosion model parameter. PN junction
characteristics, above the explosion current are linear. HSPICE/HSPICE RF
determines the slope at the explosion point. This improves simulation speed
and convergence.
See Also
BJT and Diode Examples for the path to the demo file bjtgm.sp, which uses
.OPTION EXPLI=10.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
453
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION EXPMAX
.OPTION EXPMAX
Specifies the largest exponent that you can use for an exponential before
overflow occurs.
Syntax
.OPTION EXPMAX=x
Default
80.00
Description
Use this option to specify the largest exponent that you can use for an
exponential before overflow occurs. Typical value for an IBM platform is 350.
454
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FAST
.OPTION FAST
Disables status updates for latent devices; this speeds up simulation.
Syntax
.OPTION FAST=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to set additional options, which increase simulation speed with
minimal loss of accuracy.
To speed up simulation, this option disables status updates for latent devices.
Use this option for MOSFETs, MESFETs, JFETs, BJTs, and diodes.
A device is latent if its node voltage variation (from one iteration to the next) is
less than the value of either the BYTOL control option or the BYPASSTOL
element parameter. (If FAST is on, HSPICE sets BYTOL to different values for
different types of device models.)
Besides the FAST option, you can also use the NOTOP and NOELCK options to
reduce input preprocessing time. Increasing the value of the MBYPASS or
BYTOL option, also helps simulations to run faster, but can reduce accuracy. To
see how use of FAST impacts the value settings of other options, see Appendix
B, How Options Affect other Options.
See Also
.OPTION BYTOL
.OPTION MBYPASS
.OPTION NOELCK
.OPTION NOTOP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
455
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FFT_ACCURATE
.OPTION FFT_ACCURATE
Dynamically adjusts the time step so that each FFT point is a real simulation
point in HSPICE/HSPICE RF.
Syntax
.OPTION FFT_ACCURATE=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to dynamically adjust the time step so that each FFT point is a
real simulation point. This eliminates interpolation error and provides the
highest FFT accuracy with minimal overhead in simulation time.
See Also
.OPTION ACCURATE
.OPTION SIM_ACCURACY (RF)
456
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FFTOUT
.OPTION FFTOUT
Prints 30 harmonic fundamentals.
Syntax
.OPTION FFTOUT=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to print 30 harmonic fundamentals sorted by size, THD, SNR,
and SFDR, but only if you specify a FFTOUT option and a .FFTfreq=xxx
command.
See Also
.FFT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
457
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FMAX
.OPTION FMAX
Sets the maximum frequency value of angular velocity, for poles and zeros.
Syntax
.OPTION FMAX=x
Default
1.0e+12
Description
Use this option to set the maximum frequency value of angular velocity for Pole/
Zero analysis. The units of value are in rad/sec.
See Also
.OPTION CSCAL
.OPTION FSCAL
.OPTION GSCAL
.OPTION ITLPZ
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.OPTION RITOL
.PZ
458
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FS
.OPTION FS
Decreases FS value to help circuits that have timestep convergence difficulties.
Syntax
.OPTION FS=x
Description
Use this option to decrease delta (internal timestep) by the specified fraction of
a timestep (TSTEP) for the first time point of a transient. Decreases the FS
value to help circuits that have timestep convergence difficulties. DVDT=3 uses
FS to control the timestep. Delta = FS ⋅ [ MIN ( TSTEP, DELMAX, BKPT ) ]
■
You specify DELMAX.
■
BKPT is related to the breakpoint of the source.
■
The .TRAN command sets TSTEP.
See Also
.OPTION DELMAX
.OPTION DVDT
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
459
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FSCAL
.OPTION FSCAL
Sets the frequency scale for Pole/Zero analysis.
Syntax
.OPTION FSCAL=x
Default
1e-9
Description
Use this option to set the frequency scale for Pole/Zero analysis. HSPICE
multiplies capacitances by FSCAL.
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION GSCAL
.OPTION ITLPZ
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.OPTION RITOL
.PZ
460
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION FT
.OPTION FT
Decreases delta by a specified fraction of a timestep for iteration set that does
not converge.
Syntax
.OPTION FT=x
Description
Use this option to decrease delta (the internal timestep) by a specified fraction
of a timestep (TSTEP) for an iteration set that does not converge. If DVDT=2 or
DVDT=4, FT controls the timestep.
See Also
.OPTION DVDT
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
461
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GDCPATH
.OPTION GDCPATH
Adds conductance to nodes having no DC path to ground.
Syntax
.OPTION GDCPATH[=x]
Default 1e-12
Description
Use this option to add conductance to nodes having no DC path to ground.
462
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GENK
.OPTION GENK
Automatically computes second-order mutual inductance for several coupled
inductors.
Syntax
.OPTION GENK= 0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to automatically calculate second-order mutual inductance for
several coupled inductors. The default (1) enables the calculation.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
463
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GEOSHRINK
.OPTION GEOSHRINK
Element scaling factor used with .OPTION SCALE.
Syntax
.OPTION GEOSHRINK=x
Description
Use this option as a global model to apply to all elements. In addition
to .OPTION SCALE, use this option (usually through a technology file) on top of
the existing scale option to further scale geometric element instance
parameters whose default units are meters. The final instance geometric
parameters are then be calculated as:final_dimension =
original_dimension * SCALE * GEOSHRINK
The effective scaling factor is the product of the two parameters.
The default value for both SCALE and GEOSHRINK is 1.
If a model library contains devices other that MOSFET, such as R, L, C, diode,
bjt... etc., and/or the netlist is a post-layout design with RCs, the shrink factor is
applied to all elements.
Examples
Example 1: If there is more than one geoshrink option set, only the last
geoshrink is used.
.option geoshrink=0.8
.option geoshrink=0.9
Then the final_dimension = original_dimension * SCALE * 0.9
Example 2: If there is more than one geoshrink and scale in the model
card, only the last scale and the last geoshrink are used.
.option
.option
.option
.option
scale=2u
scale=1u
geoshrink=0.8
geoshrink=0.9
Then the final_dimension = original_dimension * 1u * 0.9
See Also
.OPTION SCALE
.OPTION CMIUSRFLAG
464
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GMAX
.OPTION GMAX
Specifies the maximum conductance in parallel with a current source for .IC
and .NODESET initialization circuitry.
Syntax
.OPTION GMAX=x
Default
100.00 (mho)
Description
Use this option to specify the maximum conductance in parallel with a current
source for .IC and .NODESET initialization circuitry. Some large bipolar circuits
require you to set GMAX=1 for convergence.
See Also
.IC
.NODESET
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
465
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GMIN
.OPTION GMIN
Specifies the minimum conductance added to all PN junctions for a time sweep
in transient analysis for HSPICE/HSPICE RF.
Syntax
.OPTION GMIN=x
Default 1e-12
Description
Use this option to specify the minimum conductance added to all PN junctions
for a time sweep in transient analysis. Min value: 1e-30; Max value: 100.
See Also
.OPTION GMINDC
466
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GMINDC
.OPTION GMINDC
Specifies conductance in parallel for PN junctions and MOSFET nodes in DC
analysis.
Syntax
.OPTION GMINDC=x
Description
Use this option to specify conductance in parallel for all PN junctions and
MOSFET nodes except gates in DC analysis.GMINDC helps overcome DC
convergence problems caused by low values of off-conductance for pn
junctions and MOSFETs. You can use GRAMP to reduce GMINDC by one order
of magnitude for each step. Set GMINDC between 1e-4 and the PIVTOL value.
Min value: 1e-30; Max value: 100.
Large values of GMINDC can cause unreasonable circuit response. If your
circuit requires large values to converge, suspect a bad model or circuit. If a
matrix floating-point overflows and if GMINDC is 1.0e-12 or less, HSPICE sets
it to 1.0e-11. HSPICE manipulates GMINDC in auto-converge mode.
See Also
.DC
.OPTION GRAMP
.OPTION PIVTOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
467
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GRAMP
.OPTION GRAMP
Specifies a conductance range over which DC operating point analysis sweeps
GMINDC.
Syntax
.OPTION GRAMP=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to specify a conductance range over which the DC operating
point analysis sweeps GMINDC. HSPICE sets this value during autoconvergence. Use GRAMP with the GMINDC option to find the smallest GMINDC
value that results in DC convergence.
GRAMP specifies a conductance range over which the DC operating point
analysis sweeps GMINDC. HSPICE replaces GMINDC values over this range,
simulates each value, and uses the lowest GMINDC value where the circuit
converges in a steady state.
If you sweep GMINDC between 1e-12 mhos (default) and 1e-6 mhos, GRAMP
is 6 (value of the exponent difference between the default and the maximum
conductance limit). In this example:
■
HSPICE first sets GMINDC to 1e-6 mhos and simulates the circuit.
■
If circuit simulation converges, HSPICE sets GMINDC to 1e-7 mhos and
simulates the circuit.
■
The sweep continues until HSPICE simulates all values of the GRAMP ramp.
If the combined GMINDC and GRAMP conductance is greater than 1e-3 mho,
false convergence can occur.
Min value: 0; Max value: 1000.
See Also
.DC
.OPTION GMINDC
468
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GSCAL
.OPTION GSCAL
Sets the conductance scale for Pole/Zero analysis.
Syntax
.OPTION GSCAL=x
Default
1e+3
Description
Use this option to set the conductance scale for Pole/Zero analysis. HSPICE
multiplies the conductance and divides the resistance by GSCAL.
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.OPTION RITOL
.PZ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
469
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GSHDC
.OPTION GSHDC
Adds conductance from each node to ground when calculating the DC
operating point of the circuit.
Syntax
.OPTION GSHDC=[0|1]
Default 0
Description
Use this option to add conductance from each node to ground when calculating
the DC operating point of the circuit (.OP).
See Also
.OPTION GSHUNT
470
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION GSHUNT
.OPTION GSHUNT
Adds conductance from each node to ground.
Syntax
.OPTION GSHUNT=x
Default 0
Description
Use this option to add conductance from each node to ground. Add a small
GSHUNT to each node to help solve “timestep too small” problems caused by
either high-frequency oscillations or numerical noise.
Examples
.option
.option
.option
.option
.option
gshunt=1e-13
gshunt=1e-12
gshunt=1e-11
gshunt=1e-10
gshunt=1e-9
cshunt=1e-17
cshunt=1e-16
cshunt=5e-15
cshunt=1e-15
cshunt=1e-14
See Also
.OPTION CSHUNT
.OPTION GSHDC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
471
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBACKRYLOVDIM
.OPTION HBACKRYLOVDIM
Specifies the dimension of the Krylov subspace used by the Krylov solver.
Syntax
.OPTION HBACKRYLOVDIM=value
Default
300
Description
Use this option to specify the dimension of the Krylov subspace that the Krylov
solver uses.
The value parameter must specify an integer greater than zero. The range is 1
to infinity.
This option overrides the corresponding PAC option if specified in the netlist.
When this option is not specified in the netlist if HBACKRYLOVDIM <
HBKRYLOVDIM, then HBACKRYLOVDIM = HBKRYLOVDIM.
See Also
.HB
.OPTION HBKRYLOVDIM
472
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBACKRYLOVITER (or) HBAC_KRYLOV_ITER
.OPTION HBACKRYLOVITER (or) HBAC_KRYLOV_ITER
Specifies the number of GMRES solver iterations performed by the HB engine.
Syntax
.OPTION HBACKRYLOVITER | HBAC_KRYLOV_ITER = value
Description
Use this option to specify the number of Generalized Minimum Residual
(GMRES) solver iterations that the HB engine performs.
The value parameter must specify an integer greater than zero. The range is 1
to infinity.
This option overrides the corresponding PAC option if specified in the netlist.
See Also
.HBAC
.OPTION HBKRYLOVDIM
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
473
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBACTOL
.OPTION HBACTOL
Specifies the absolute error tolerance for determining convergence.
Syntax
.OPTION HBACTOL=value
Default
1.e-8
Description
Use this option to specify the absolute error tolerance for determining
convergence. The value parameter must specify a real number greater than
zero. The range is 1.e-14 to infinity.
This option overrides the corresponding PAC option if specified in the netlist.
When this option is not specified in the netlist if HBACTOL > HBTOL, then
HBACTOL = HBTOL.
See Also
.HB
.OPTION HBTOL
474
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBCONTINUE
.OPTION HBCONTINUE
Specifies whether to use the sweep solution from the previous simulation as
the initial guess for the present simulation.
Syntax
.OPTION HBCONTINUE= 0|1
Default
1
Description
Use this option to specify whether to use the sweep solution from the previous
simulation as the initial guess for the present simulation.
■
HBCONTINUE=1 Use solution from previous simulation as the initial guess.
■
HBCONTINUE=0: Start each simulation in a sweep from the DC solution.
See Also
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
475
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBFREQABSTOL
.OPTION HBFREQABSTOL
Specifies the maximum absolute change in frequency between solver iterations
for convergence.
Syntax
.OPTION HBFREQABSTOL=value
Default 1Hz
Description
Use this option to specify the maximum absolute change in frequency between
solver iterations for convergence.
This option is an additional convergence criterion for oscillator analysis.
See Also
.HBOSC
476
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBFREQRELTOL
.OPTION HBFREQRELTOL
Specifies the maximum relative change in frequency between solver iterations
for convergence.
Syntax
.OPTION HBFREQRELTOL=value
Description
Use this option to specify the maximum relative change in frequency between
solver iterations for convergence.
This option is an additional convergence criterion for oscillator analysis.
See Also
.HBOSC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
477
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HB_GIBBS
.OPTION HB_GIBBS
Option for HBTRAN output to minimize Gibbs’ phenonema.
Syntax
.OPTION HB_GIBBS=n
Default
0
Description
Minimize any Gibbs' phenomenon that may occur in transforming a squarewave signal from the frequency domain to the time domain. < n >=0 (defaults to
zero, which is equivalent to not using it at all). The result is that the HBTRAN
N
waveforms are filtered by a ( sin c ( x ) ) function before being transformed to the
time domain via FFT. This option applies only to single-tone output.
Examples
.option hb_gibbs = 2
...
.print hbtran v(2)
See Also
The HSPICE User Guide: RF Analysis, Minimizing Gibbs Phenomenon
478
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBJREUSE
.OPTION HBJREUSE
Controls when to recalculate the Jacobson matrix.
Syntax
.OPTION HBJREUSE=0|1
Default
Conditional, see below
Description
Use this option to control when to recalculate the Jacobson matrix.
■
HBJREUSE=0: Recalculates the Jacobian matrix at each iteration. This is
the default if HBSOLVER=1.
■
HBJREUSE=1: Reuses the Jacobian matrix for several iterations if the error
is sufficiently reduced. This is the default if HBSOLVER=0.
See Also
.HB
.OPTION HBSOLVER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
479
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBJREUSETOL
.OPTION HBJREUSETOL
Determines when to recalculate Jacobian matrix if HBJREUSE=1.0.
Syntax
.OPTION HBJREUSETOL=value
Description
Determines when to recalculate Jacobian matrix (if HBJREUSE=1.0).
This is the percentage by which HSPICE RF must reduce the error from the last
iteration so you can use the Jacobian matrix for the next iteration. The value
parameter must specify a real number between 0 and 1.
See Also
.HB
.OPTION HBJREUSE
480
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBKRYLOVDIM
.OPTION HBKRYLOVDIM
Specifies the dimension of the subspace used by the Krylov solver.
Syntax
.OPTION HBKRYLOVDIM=value
Description
Use this option to specify the dimension of the Krylov subspace that the Krylov
solver uses.
The value parameter must specify an integer greater than zero.
See Also
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
481
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBKRYLOVTOL
.OPTION HBKRYLOVTOL
Specifies the error tolerance for the Krylov solver.
Syntax
.OPTION HBKRYLOVTOL=value
Default
0.01
Description
Use this option to specify the error tolerance for the Krylov solver.
The value parameter must specify a real number greater than zero.
See Also
.HB
482
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBKRYLOVMAXITER (or) HB_KRYLOV_MAXITER
.OPTION HBKRYLOVMAXITER (or)
HB_KRYLOV_MAXITER
Specifies the maximum number of GMRES solver iterations performed by the
HB engine.
Syntax
.OPTION HBKRYLOVMAXITER | HB_KRYLOV_MAXITER =value
Default
500
Description
Use this option to specify the maximum number of Generalized Minimum
Residual (GMRES) solver iterations that the HB engine performs.
Analysis stops when the number of iterations reaches this value.
See Also
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
483
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBLINESEARCHFAC
.OPTION HBLINESEARCHFAC
Specifies the line search factor.
Syntax
.OPTION HBLINESEARCHFAC=value
Default
0.35
Description
Use this option to specify the line search factor.
If Newton iteration produces a new vector of HB unknowns with a higher error
than the last iteration, then scale the update step by this value and try again.
The value parameter must specify a real number between 0 and 1.
See Also
.HB
484
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBMAXITER (or) HB_MAXITER
.OPTION HBMAXITER (or) HB_MAXITER
Specifies the maximum number of Newton-Raphson iterations performed by
the HB engine.
Syntax
.OPTION HBMAXITER | HB_MAXITER=value
Default
10000
Description
Use this option to specify the maximum number of Newton-Raphson iterations
that the HB engine performs.
Analysis stops when the number of iterations reaches this value.
See Also
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
485
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBOSCMAXITER (or) HBOSC_MAXITER
.OPTION HBOSCMAXITER (or) HBOSC_MAXITER
Specifies the maximum number of outer-loop iterations for oscillator analysis.
Syntax
.OPTION HBOSCMAXITER | HBOSC_MAXITER=value
Default
10000
Description
Use this option to specify the maximum number of outer-loop iterations for
oscillator analysis.
See Also
.HBOSC
486
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBPROBETOL
.OPTION HBPROBETOL
Searches for a probe voltage at which the probe current is less than the
specified value.
Syntax
.OPTION HBPROBETOL=value
Default
1.e-9
Description
Use this option to cause oscillator analysis to try to find a probe voltage at
which the probe current is less than the specified value.
This option defaults to the value of the HBTOL option, which defaults to 1.e-9.
See Also
.HBOSC
.OPTION HBTOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
487
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBSOLVER
.OPTION HBSOLVER
Specifies a preconditioner for solving nonlinear circuits.
Syntax
.OPTION HBSOLVER=0|1|2
Default
1
Description
Use this option to specify a preconditioner for solving nonlinear circuits.
■
HBSOLVER=0: Invokes the direct solver.
■
HBSOLVER=1 Invokes the matrix-free Krylov solver.
■
HBSOLVER=2: Invokes the two-level hybrid time-frequency domain solver.
See Also
.HBOSC
.OPTION HBJREUSE
488
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBTOL
.OPTION HBTOL
Specifies the absolute error tolerance for determining convergence.
Syntax
.OPTION HBTOL=value
Description
Use this option to specify the absolute error tolerance for determining
convergence.
The value parameter must specify a real number greater than zero.
See Also
.HB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
489
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBTRANFREQSEARCH
.OPTION HBTRANFREQSEARCH
Specifies the frequency source for the HB analysis of a ring oscillator.
Syntax
.OPTION HBTRANFREQSEARCH=[1|0]
Default
1
Description
Use this option to specify the frequency source for the HB analysis of a ring
oscillator.
■
HBTRANFREQSEARCH=1: HB analysis calculates the oscillation frequency
from the transient analysis
■
HBTRANFREQSEARCH=0: HB analysis assumes that the period is 1/f, where
f is the frequency specified in the tones description.
See Also
.HB
.HBOSC
.OPTION HBTOL
490
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBTRANINIT
.OPTION HBTRANINIT
Selects transient analysis for initializing all state variables for HB analysis of a
ring oscillator.
Syntax
.OPTION HBTRANINIT=time
Description
Use this option to cause HB to use transient analysis to initialize all state
variables for HB analysis of a ring oscillator.
The time parameter is defined by when the circuit has reached (or is near)
steady-state. The default is 0.
See Also
.HB
.HBOSC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
491
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBTRANPTS
.OPTION HBTRANPTS
Specifies the number of points per period for converting time-domain data
results into the frequency domain for HB analysis of a ring oscillator.
Syntax
.OPTION HBTRANPTS=npts
Default
4*nh
Description
Use this option to specify the number of points per period for converting the
time-domain data results from transient analysis into the frequency domain for
HB analysis of a ring oscillator.
The npts parameter must be set to an integer greater than 0. The units are in
nharms (nh).
This option is relevant only if you set .OPTION HBTRANINIT. You can specify
either .OPTION HBTRANPTS or .OPTION HBTRANSTEP, but not both.
See Also
.HB
.HBOSC
.OPTION HBTRANINIT
.OPTION HBTRANSTEP
492
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HBTRANSTEP
.OPTION HBTRANSTEP
Specifies transient analysis step size for the HB analysis of a ring oscillator.
Syntax
.OPTION HBTRANSTEP=stepsize
Description
Use this option to specify transient analysis step size for the HB analysis of a
ring oscillator.
The stepsize parameter must be set to a real number. The default is 1/
(4*nh*f0), where nh is the nharms value and f0 is the oscillation frequency.
This option is relevant only if you set .OPTION HBTRANINIT.
Note:
You can specify either .OPTION HBTRANPTS or .OPTION
HBTRANSTEP, but not both.
See Also
.HB
.HBOSC
.OPTION HBTRANINIT
.OPTION HBTRANPTS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
493
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HIER_DELIM
.OPTION HIER_DELIM
Replaces the caret delimiter with a period (for output control only) when used
for HSPICE/ADE only.
Syntax
.OPTION HIER_DELIM= 0|1
Default
Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use .OPTION HIER_DELIM to change the hierarchy delimiter from a caret (^)
to a period (.) only with for the HSPICE integration to Cadence® Virtuoso®
ADE. When .OPTION HIER_DELIM=1, a caret (^) is changed to a period(.).
This option works with .OPTION PSF and .OPTION ARTIST.
■
0: Maintains the caret.
■
1: Replaces the caret with a period.
See Also
.OPTION ARTIST
.OPTION PSF
494
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HIER_SCALE
.OPTION HIER_SCALE
Uses the parameter S to scale subcircuits.
Syntax
.OPTION HIER_SCALE=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option so you can use the parameter S to scale subcircuits.
■
0 Interprets S as a user-defined parameter.
■
1 Interprets S as a scale parameter.
This option enables you to selectively scale the required instance. See the
example below.
Examples
Assume you have an encrypted subcircuit from an IP vendor A which has
.option SCALE=1e-6 defined. You have another encrypted subcircuit (from
another IP vendor B), which has the units defined as microns and does not
need to be scaled. When you simulate the circuit, HSPICE applies the SCALE
option globally and the subcircuit from IP vendor B is scaled again. You can
selectively apply the SCALE option so that this does not happen, as follows:
* Top level netlist
.option hier_scale=1
.include "subckt_a.inc" $ subcircuit from IP vendor A
.include "subckt_b.inc" $ subcircuit from IP vendor B
vin in 0 5
x1 in 2 subckt_a $ uses .option scale=1e-6 defined in subckt_a.inc
file
x2 2 0 subckt_b S=1e6 $ scale option is not required
.tran 100p 10n
.end
The subckt_a.inc file has .option scale=1u defined and this is applied
globally. When .option hier_scale=1 is used and the subcircuit instance,
X2 contains S=1e6, the global scaling is offset.If W=10u is used in subcircuit
instance X2 and hier_scale is used, then:
W="10u*SCALE*S"="10u*1u*1e6"=10u
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
495
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION HIER_SCALE
If W=10 is used in subcircuit instance X1 and “S” is not used, then only the
global .option SCALE=1e-6 is applied and the value of W is 10u.
496
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION IC_ACCURATE
.OPTION IC_ACCURATE
Improves the accuracy of the .IC command.
Syntax
.OPTION IC_ACCURATE=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
When .OPTION IC_ACCURATE=1 the .IC command accuracy is increased
for cases requiring tighter precision (for example, when the GMAX value is too
large) than is used to set the maximum conductance in parallel with a current
source for .IC and .NODESET initialization circuitry. The option overrides the
approximating method used by the .IC command with only slight performance
cost. If the option is not set or it equals 0, then the default .IC method is used.
See Also
.IC
.OPTION GMAX
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
497
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ICSWEEP
.OPTION ICSWEEP
Saves the current analysis result of a parameter or temperature sweep as the
starting point in the next analysis.
Syntax
.OPTION ICSWEEP=0|1
Default
1
Description
Use this option to save the current analysis result of a parameter or
temperature sweep as the starting point in the next analysis in the sweep.
498
■
If ICSWEEP=1, the next analysis uses the current results.
■
If ICSWEEP=0, the next analysis does not use the results of the current
analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION IMAX
.OPTION IMAX
Specifies the maximum timestep in timestep algorithms for transient analysis.
Syntax
.OPTION IMAX=x
Description
Use this option to specify the maximum timestep in algorithms for transient
analysis.IMAX sets the maximum iterations to obtain a convergent solution at a
timepoint. If the number of iterations needed is greater than IMAX, the internal
timestep (delta) decreases by a factor equal to the FT transient control option.
The new timestep calculates a new solution. IMAX also works with the IMIN
transient control option. IMAX is the same as ITL4.
See Also
.OPTION FT
.OPTION IMIN
.OPTION ITL4
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
499
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION IMIN
.OPTION IMIN
Specifies the minimum timestep in timestep algorithms for transient analysis.
Syntax
.OPTION IMIN=x
Description
Use this option to specify the minimum number of iterations required to obtain
convergence for transient analysis. If the number of iterations is less than
IMIN, the internal timestep (delta) doubles.
Use this option to decrease simulation times in circuits where the nodes are
stable most of the time (such as digital circuits). If the number of iterations is
greater than IMIN, the timestep stays the same unless the timestep exceeds
the IMAX option. IMIN is the same as ITL3.
See Also
.OPTION IMAX
.OPTION ITL3
500
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION INGOLD
.OPTION INGOLD
Controls whether HSPICE prints *.lis file output in exponential form or
engineering notation in HSPICE/HSPICE RF.
Syntax
.OPTION INGOLD=[0|1|2]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Argument
Description
INGOLD=0
Engineering Format; defaults 1.234K, 123M
INGOLD=1
G Format (fixed and exponential); defaults 1.234e+03, .123
INGOLD=2
E Format (exponential SPICE); defaults 1.234e+03, .123e-1
Description
Use this option to control if HSPICE prints output in exponential form (scientific
notation) or engineering notation. Engineering notation provides two to three
extra significant digits and aligns columns to facilitate comparison, as:
F=1e-15
M=1e-3
P=1e-12
K=1e3
N=1e-9
X=1e6
U=1e-6
G=1e9
HSPICE RF prints variable values in engineering notation by default. To use the
exponential form, specify .OPTION INGOLD=1 or 2. To print variable values in
exponential form, specify .OPTION INGOLD=1 or 2.
.OPTION INGOLD does not control the number format in measure files(*.mt#/
*.ms#/*.ma#). If you specify a measure output file using .OPTION MEASFORM,
HSPICE automatically resets an INGOLD=0 setting to INGOLD=1, which allows
the measure file to be imported to Excel when .OPTION MEASFORM=1.
Examples
.OPTION INGOLD=2
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
501
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION INGOLD
See Also
.OPTION MEASDGT
.OPTION MEASFORM
502
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION INTERP
.OPTION INTERP
Limits output to only the .TRAN timestep intervals for post-analysis tools.
Syntax
.OPTION INTERP=0|1
Default Value if option is not specified in the netlist: 0 (engineering notation)
Value if option name is specified without a corresponding value: 1
Description
Use to limit output for post-analysis tools to only the .TRAN timestep intervals
for some post-analysis tools. This option can be used to reduce the size of the
post-processing output. By default, HSPICE outputs data at internal timepoints.
In some cases, INTERP produces a much larger design .tr# file, especially for
smaller timesteps, and it also leads to longer runtime.
Note:
Since HSPICE uses the post-processing output to compute the
.MEASURE command results, interpolation errors result if you
use the INTERP option and your netlist also
contains .MEASURE commands. Using the INTERP option with
.MEASURE commands is not recommended.
When you run data-driven transient analysis (.TRAN DATA) in an optimization
routine, HSPICE forces INTERP=1. All measurement results are at the time
points specified in the data-driven sweep. To measure only at converged
internal timesteps (for example, to calculate the AVG or RMS), set ITRPRT=1.
See Also
.OPTION ITRPRT
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
503
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION IPROP
.OPTION IPROP
Controls whether to treat all of the circuit information as IP protected.
Syntax
.OPTION IPROP 0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use to control whether to treat all of the circuit information as IP protected and
not output this information during simulation.
504
■
0= Output information (IP not protected)
■
1=Do not output information (IP protected)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITL1
.OPTION ITL1
Specifies the maximum DC iteration limit.
Syntax
.OPTION ITL1=n
Description
Use this option to specify the maximum DC iteration limit. Increasing this value
rarely improves convergence in small circuits. Values as high as 400 have
resulted in convergence for some large circuits with feedback (such as
operational amplifiers and sense amplifiers). However, most models do not
require more than 100 iterations to converge.
See Also
.DC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
505
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITL2
.OPTION ITL2
Specifies the iteration limit for the DC transfer curve.
Syntax
.OPTION ITL2=n
Description
Use this option to specify the iteration limit for the DC transfer curve. Increasing
this limit improves convergence only for very large circuits.
See Also
.DC
506
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITL3
.OPTION ITL3
Specifies minimum timestep in timestep algorithms for transient analysis.
Syntax
.OPTION ITL3=x
Description
Use this option to specify the minimum timestep in timestep algorithms for
transient analysis.ITL3 is the minimum number of iterations required to obtain
convergence. If the number of iterations is less than ITL3, the internal timestep
(delta) doubles.
Use this option to decrease simulation times in circuits where the nodes are
stable most of the time (such as digital circuits). If the number of iterations is
greater than IMIN, the timestep stays the same unless the timestep exceeds
the IMAX option. ITL3 is the same as IMIN.
See Also
.OPTION IMAX
.OPTION IMIN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
507
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITL4
.OPTION ITL4
Specifies maximum timestep in timestep algorithms for transient analysis in
HSPICE/HSPICE RF.
Syntax
.OPTION ITL4=x
Default
8
Description
Use this option to specify the maximum timestep in timestep algorithms for
transient analysis.ITL4 sets the maximum iterations to obtain a convergent
solution at a timepoint. If the number of iterations needed is greater than ITL4,
the internal timestep (delta) decreases by a factor equal to the FT transient
control option. HSPICE uses the new timestep to calculate a new solution.
ITL4 also works with the IMIN transient control option. For HSPICE, ITL4 is
the same as IMAX.
See Also
.OPTION FT
.OPTION IMAX
.OPTION IMIN
508
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITL5
.OPTION ITL5
Sets an iteration limit for transient analysis.
Syntax
.OPTION ITL5=x
Default 0 (infinite number of iterations)
Description
Use this option to set an iteration limit for a transient analysis. If a circuit uses
more than ITL5 iterations, the program prints all results up to that point.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
509
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITLPTRAN
.OPTION ITLPTRAN
Controls iteration limit used in the final try of the pseudo-transient method.
Syntax
.OPTION ITLPTRAN=x
Default
30
Description
Use this option to control the iteration limit used in the final try of the pseudotransient method in OP or DC analysis. If a simulation fails in the final try of the
pseudo-transient method, provide a higher value.
See Also
.DC
.OP
510
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITLPZ
.OPTION ITLPZ
Sets the iteration limit for pole/zero analysis.
Syntax
.OPTION ITLPZ=x
Default
100
Description
Use this option to set the iteration limit for pole/zero analysis.
See Also
.OPTION CSCAL
.OPTION GSCAL
.PZ
.OPTION FMAX
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
511
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION ITRPRT
.OPTION ITRPRT
Enables printing of output variables at their internal time points.
Syntax
.OPTION ITRPRT 0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to enable printing of output variables at their internal time
points.
When set to 1, HSPICE prints output variables at their internal transient
simulation time points. In addition, if you use the -html option when invoking
HSPICE, then HSPICE prints the values to a separate file (*.printtr0).
512
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION IVTH
.OPTION IVTH
Invokes a constant-current threshold voltage probing and characterization
function for BSIM4 models.
Syntax
.OPTION IVTH=val | IVTHN=val | IVTHP=val
Description
Specifies the ivth constant drain terminal current density, to be multiplied by the
ratio of transistor width (W) and length (L). The value must be greater than zero
to enable the function; the IVTH option should always be set to a positive value
for both PMOS and NMOS.
.OPTION IVTH has been enhanced to support HSPICE BSIM4 (level 54),
BSIMSOI4.x (level 70) and PSP (level 69). .OPTION IVTHN and IVTHP
support NMOS and PMOS, respectively.
Note:
The val should be a constant.
In OP analysis, a constant current based vth is reported in the OP output. In
addition, the element region operation check and Vod output are based on the
new vth. During transient or DC analysis, a template output of LX142
accesses the new vth value.LX142(m*) or ivth(m*) could be used for the
new vth output. This methodology is based on the monotony Id/Vgs curve.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
513
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION KCLTEST
.OPTION KCLTEST
Activates the KCL (Kirchhoff’s Current Law) test.
Syntax
.OPTION KCLTEST=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to activate the KCL test. This increases simulation time,
especially for large circuits, but checks the solution with a high degree of
accuracy.
If you set this value to 1, HSPICE sets these options:
■
Sets RELMOS and ABSMOS options to 0 (off).
■
Sets ABSI to 1e-6 A.
■
Sets RELI to 1e-6.
To satisfy the KCL test, each node must satisfy this condition:
Σi b < RELI ⋅ Σ i b + ABSI
In this equation, the ibs are the node currents.
See Also
.OPTION ABSI
.OPTION ABSMOS
.OPTION RELI
.OPTION RELMOS
514
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION KLIM
.OPTION KLIM
Sets the minimum mutual inductance.
Syntax
.OPTION KLIM=x
Description
Use this option to set the minimum mutual inductance below which automatic
second-order mutual inductance calculation no longer proceeds. KLIM is
unitless (analogous to coupling strength, specified in the K-element). Typical
KLIM values are between .5 and 0.0.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
515
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LA_FREQ
.OPTION LA_FREQ
Specifies the upper frequency for which accuracy must be preserved.
Syntax
.OPTION LA_FREQ=value
Default
1GHz
Description
Use this option to specify the upper frequency for which accuracy must be
preserved.
The value parameter specifies the upper frequency for which the PACT
algorithm must preserve accuracy. If value is 0, the algorithm drops all
capacitors because only DC is of interest.
The maximum frequency required for accurate reduction depends on both the
technology of the circuit and the time scale of interest. In general, the faster the
circuit, the higher the maximum frequency.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: Simulation and Analysis.
See Also
.OPTION SIM_LA
.OPTION LA_TIME
516
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LA_MAXR
.OPTION LA_MAXR
Specifies the maximum resistance for linear matrix reduction.
Syntax
.OPTION LA_MAXR=value
Default
1e15 ohms
Description
Use this option to specify the maximum resistance for linear matrix reduction.
The value parameter specifies the maximum resistance preserved in the
reduction. The linear matrix reduction process assumes that any resistor
greater than value has an infinite resistance and drops the resistor after
reduction is completed.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: Simulation and Analysis.
See Also
.OPTION SIM_LA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
517
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LA_MINC
.OPTION LA_MINC
Specifies the minimum capacitance for linear matrix reduction.
Syntax
.OPTION LA_MINC=val
Default 1e-16 farads
Description
Removes any capacitor in the original netlist less than the value of LA_MINC
prior to reduction. For additional information, see “Linear Acceleration” in the
HSPICE User Guide: Simulation and Analysis.
See Also
.OPTION SIM_LA
.OPTION LA_FREQ
.OPTION LA_MAXR
.OPTION LA_TIME
.OPTION LA_TOL
518
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LA_TIME
.OPTION LA_TIME
Specifies the minimum time for which accuracy must be preserved.
Syntax
.OPTION LA_TIME=value
Description
Use this option to specify the minimum time for which accuracy must be
preserved. The value parameter specifies the minimum switching time for
which the PACT algorithm preserves accuracy.
Waveforms that occur more rapidly than the minimum switching time are not
accurately represented.
This option is simply an alternative to .OPTION LA_FREQ. The default is
equivalent to setting LA_FREQ=1GHz.
Note:
Higher frequencies (smaller times) increase accuracy, but only
up to the minimum time step used in HSPICE.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: Simulation and Analysis.
Examples
For a circuit having a typical rise time of 1ns, either set the maximum frequency
to 1 GHz, or set the minimum switching time to 1ns:
.OPTION LA_FREQ=1GHz
-or.OPTION LA_TIME=1ns
However, if spikes occur in 0.1ns, HSPICE does not accurately simulate them.
To capture the behavior of the spikes, use:
.OPTION LA_FREQ=10GHz
-or.OPTION LA_TIME=0.1ns
See Also
.OPTION SIM_LA
.OPTION LA_FREQ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
519
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LA_TOL
.OPTION LA_TOL
Specifies the error tolerance for the PACT algorithm.
Syntax
.OPTION LA_TOL=value
Default
0.05
Description
Use this option to specify the error tolerance for the PACT algorithm.
The value parameter must specify a real number between 0.0 and 1.0.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: Simulation and Analysis.
See Also
.OPTION SIM_LA
520
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LENNAM
.OPTION LENNAM
Specifies maximum name length for printing operating point analysis results.
Syntax
.OPTION LENNAM=x
Default 16 (characters)
Description
Use this option to specify the maximum length of names in the printout of
operating point analysis results. The maximum value is 1024. .OPTION
LENNAME prints the full related name of the transistor in the noise tables and
OP tables.
Examples
...
.OPTIONS POST=1 LENNAM=40
...
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
521
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LIMPTS
.OPTION LIMPTS
Specifies the number of points to print in AC analysis.
Syntax
.OPTION LIMPTS=x
Default
2001
Description
Use this option to specify the number of points to print or plot in AC analysis.
You do not need to set LIMPTS for a DC or transient analysis. HSPICE spools
the output file to disk.
See Also
.AC
.DC
.TRAN
522
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LIMTIM
.OPTION LIMTIM
Specifies the amount of CPU time reserved to generate prints.
Syntax
.OPTION LIMTIM=x
Default 2 (seconds)
Description
Use this option to specify the amount of CPU time reserved to generate prints
and plots if a CPU time limit (CPTIME=x) terminates simulation. Default is
normally sufficient for short printouts.
See Also
.OPTION CPTIME
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
523
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LISLVL
.OPTION LISLVL
Controls whether of not HSPICE suppresses the circuit number to circuit
hierarchy information in the listing file.
Syntax
LISLVL=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
LISLVL=0 prints the circuit name directory information in the .lis file.If the
value is 1, the circuit number and circuit hierarchy information is not output to
the .lis file.
524
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LIS_NEW
.OPTION LIS_NEW
Enables streamlining improvements to the *.lis file.
Syntax
.OPTION LIS_NEW=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use .OPTION LIS_NEW to activate several streamlining improvements to the
*.lis file as noted below. A value of 0 disables the following functions. A value of
1 enables the following:
■
Moves .PRINT data and .NOISE analysis data to separate files,
■
Suppresses operating point node voltage table that exists in the *.ic# file.
■
Prints loading information for input files.
■
Invokes console printing of simulation progress percentage.
■
Adds a convergence status update to *.lis.
■
Increments every 10% of analysis update to *.lis.
■
Reports analysis output file with analysis-specific format.
■
Prints Improved format of circuit statistics information.
■
Operating point analysis information is separated to file if .OP is used in
netlist (LIS_NEW=1 automatically sets .OPTION OPFILE=1).
■
Model related information is suppressed(lis_new=1 automatically sets
.OPTION NOMOD=1).Circuit hierarchy to number mapping information is
not printed to *.lis file and .OPTION LISLVL becomes nullified with usage
of LIS_NEW=1.
See Also
.OPTION LIST
.LIB
.NOISE
.OPTION LISLVL
.OPTION NOMOD.OPTION OPFILE
.OP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
525
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LIST
.OPTION LIST
Prints a list of netlist elements, node connections, and values for components,
voltage and current sources, parameters, and more.
Syntax
.OPTION LIST=0|1|2|3
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option as follows:
Value
Alias
Description
0
NONE
None of below supported
1
ALL
Print circuit element summary table and parameter definitions
2
ELEMENT
Print circuit element summary table only
3
PARAMETER
Print circuit parameter definitions only
The LIST option also prints effective sizes of elements and key values.
Note:
This option is suppressed by the BRIEF option.
See Also
.OPTION BRIEF
.OPTION LIS_NEW
.OPTION UNWRAP
.OPTION VFLOOR
526
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LOADHB
.OPTION LOADHB
Loads state variable information from a specified file.
Syntax
.OPTION LOADHB=’filename’
Description
Use this option to load the state variable information contained in the specified
file. These values are used to initialize the HB simulation.
See Also
.HB
.OPTION SAVEHB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
527
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LOADSNINIT
.OPTION LOADSNINIT
Loads the operating point saved at the end of Shooting Newton analysis
initialization.
Syntax
.OPTION LOADSNINIT="filename"
Description
Use this option to load the operating point file saved at the end of SN
initialization, which is used as initial conditions for the Shooting-Newton
method.
528
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LSCAL
.OPTION LSCAL
Sets the inductance scale for Pole/Zero analysis.
Syntax
.OPTION LSCAL=x
Default
1e+6
Description
Use this option to set the inductance scale for Pole/Zero analysis. HSPICE
multiplies inductance by LSCAL.
Note:
Scale factors must satisfy the following
relations: GSCAL = CSCAL ⋅ FSCAL
1
GSCAL = --------------------------------------------LSCAL ⋅ FSCAL
If you change scale factors, you might need to modify the initial
Muller points, (X0R, X0I), (X1R, X1I) and (X2R, X2I), even
though HSPICE internally multiplies the initial values by (1.0e-9/
GSCAL).
The three complex starting-trial points, in the Muller (x1R,X1I) algorithm for
pole/zero analysis are listed below with their defaults. HSPICE multiplies these
initial points, and FMAX, by FSCAL.
Starting-Trial Points
Defaults
.OPTION (X0R,X0I)
X0R=-1.23456e6
X0I=0.0
.OPTION (X1R,X1I)
X1R=1.23456e5
X1I=0.0
.OPTION (X2R,X21)
X2R=+1.23456e6
X2I=0.0
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION ITLPZ
.OPTION PZABS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
529
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LSCAL
.OPTION PZTOL
.OPTION RITOL
.OPTION (X0R,X0I)
.OPTION (X1R,X1I)
.OPTION (X2R,X21)
.PZ
530
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION LVLTIM
.OPTION LVLTIM
Selects the timestep algorithm for transient analysis.
Syntax
.OPTION LVLTIM=[1|2|3]|4]
Default
1
Description
Use this option, (levels 1-3, only) to select the timestep algorithm for transient
analysis.
■
LVLTIM=1 (default) uses the DVDT timestep control algorithm.
■
LVLTIM=2 uses the local truncation error (LTE) timestep control method.
You can apply LVLTIM=2 to the TRAP method.
■
LVLTIM=3 uses the DVDT timestep control method with timestep reversal.
■
LVLTIM=4 is invalid if set by user; it is invoked by the RUNLVL option only
to enhance the LTE time step control method used by the latest RUNLVL
algorithm.
The local truncation algorithm LVLTIM=2 (LTE) provides a higher degree of
accuracy than LVLTIM=1 or 3 (DVDT). If you use this option, errors do not
propagate from time point to time point, which can result in an unstable
solution.
Selecting the GEAR method changes the value of LVLTIM to 2 automatically.
For information on how LVLTIM values impact other options, see Appendix B,
How Options Affect other Options.
See Also
.OPTION CHGTOL
.OPTION DVDT
.OPTION FS
.OPTION FT
.OPTION RELQ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
531
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MACMOD
.OPTION MACMOD
Enables HSPICE MOSFET to access the subcircuit definition when there is no
matching model reference or enables an HSPICE X-element to access the
model reference when there is no matching subcircuit definition.
Syntax
.OPTION MACMOD=[1|2|3|0]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
The following describes .OPTION MACMOD characteristics:
■
When macmod=1, HSPICE seeks a subckt definition for the M*** element if
no model reference exists. The desired subckt name must match (case
insensitive) the mname field in the M*** instance command. In addition, the
number of terminals of the subckt must match with the M*** element
referencing it; otherwise HSPICE exits the simulation based on no definition
for the M*** element. In addition, the M instance can call Verilog-A models
when macmod=1.
■
When macmod=2, HSPICE seeks a MOSFET model definition when it
cannot find a matching subckt or Verilog-A definition for an X-element. The
targeted MOSFET MODEL card could be either an HSPICE built-in
MOSFET model or CMI MOSFET model. If the model card that matched the
X-element reference name is not a type of MOSFET model, the simulator
exits and displays an error message indicating that the reference is not
found.
■
When macmod=3, HSPICE enables the same features as when macmod=1.
HSPICE seeks a .subckt definition for an M-element if there is no
matching model reference; HSPICE seeks a .model MOSFET definition for
an X-element if there is no matching .subckt or Verilog-A definition. Usage
considerations and limitations remain the same for both features,
respectively.
If .OPTION TMIFLAG=1, .OPTION MACMOD automatically equals 3.
Note:
532
When MACMOD=2 or 3, for the X-element that maps to an Melement, if it has an instance parameter named ‘Multi’ (case
insensitive), then ‘Multi’ is used as an alias for the ‘M’ factor (the
M multiply parameter).
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MACMOD
When macmod=0: if there is no .option MACMOD in the input files or
MACMOD=0, then neither of the features is enabled. HSPICE ignores the option
MACMOD when any value other than 1|2|3|0 is set.The MACMOD option is a
global option; if there are multiple MACMOD options in one simulation, HSPICE
uses the value of the last MACMOD option.
For examples and detailed discussion, see MOSFET Element Support
Using .OPTION MACMOD in the HSPICE User Guide: Simulation and
Analysis.
See Also
.OPTION TMIFLAG
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
533
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MAXAMP
.OPTION MAXAMP
Sets the maximum current through voltage-defined branches.
Syntax
.OPTION MAXAMP=x
Description
Use this option to set the maximum current through voltage-defined branches
(voltage sources and inductors). If the current exceeds the MAXAMP value,
HSPICE reports an error.
534
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MAXORD
.OPTION MAXORD
Specifies the maximum order of integration for the GEAR method.
Syntax
.OPTION MAXORD=[1|2|3]
Description
Use this option to specify the maximum order of integration for the GEAR
method. When the GEAR method is used, based on the circuit type, HSPICE/
HSPICE RF automatically switches the GEAR order on the fly. If this option is
not specifically set, HSPICE automatically selects the BDF or GEAR integration
method based on circuit type when METHOD=GEAR.
The value of the parameter can be either 1, 2, or 3:
■
MAXORD=1 selects the first-order GEAR (Backward-Euler) integration (and
prohibits GEAR from switching to BDF).
■
MAXORD=2 selects the second-order GEAR (Gear-2), which is more stable
and accurate than MAXORD=1.
■
MAXORD=3 selects the third-order or high GEAR (Gear-3), which is most
accurate, since it uses 3 previous time points to estimate the next time point.
Examples
This example selects the Backward-Euler integration method.
.OPTION MAXORD=1 METHOD=GEAR
See Also
.OPTION METHOD
.OPTION RUNLVL (HSPICE)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
535
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MAXWARNS
.OPTION MAXWARNS
Specifies maximum number of safe operating area (SOA) warning messages.
Syntax
.OPTION MAXWARNS=n
Default 5
Description
Use this option to specify the maximum number of SOA warning messages
when terminal voltages of a device (MOSFET, BJT, Diode, Resistor, Capacitor
etc…) exceed a safe operating area. This option is used with .OPTION WARN.
See Also
.OPTION WARN
Safe Operating Area (SOA) Warnings
536
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MBYPASS
.OPTION MBYPASS
Computes the default value of the BYTOL control option.
Syntax
.OPTION MBYPASS=x
Description
Use this option to calculate the default value of the BYTOL control option:
Also multiplies the RELV voltage tolerance. Set MBYPASS to about 0.1 for
precision analog circuits.
■
Default is 1 for DVDT=0, 1, 2, or 3.
■
Default is 2 for DVDT=4.
See Also
.OPTION BYTOL
.OPTION DVDT
.OPTION RELV
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
537
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MCBRIEF
.OPTION MCBRIEF
Controls how HSPICE outputs Monte Carlo parameters.
Syntax
.OPTION MCBRIEF=0|1|2|3
Default
0
Description
Use this option to control how HSPICE outputs Monte Carlo parameters:
■
MCBRIEF=0: Outputs all Monte Carlo parameters
■
MCBRIEF=1: Suppresses Monte Carlo parameters in *.mt# and *.lis files;
also suppresses generation of *.mc?#, *.mpp#, *.annotate, and *.corner
files.
■
MCBRIEF=2: Outputs the Monte Carlo parameters into a .lis file only.
■
MCBRIEF=3: Outputs the Monte Carlo parameters into the measure files
only.
Note that this option only works for parameters defined in a netlist, and not for
measurement results.
538
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MEASDGT
.OPTION MEASDGT
Formats the .MEASURE command output of significant digits in both the listing
file and the .MEASURE output files.
Syntax
.OPTION MEASDGT=x
Default
4
Description
Use this option to format the .MEASURE command output’s significant digits in
both the listing file and the .MEASURE output files (.ma0, .mt0, .ms0, and so
on).
The value of x is typically between 1 and 7 significant digits, although you can
set it as high as 10.
Use MEASDGT with .OPTION INGOLD=x to control the output data format.
Examples
For example, if MEASDGT=5, then .MEASURE displays numbers as:
■
Five decimal digits for numbers in scientific notation.
■
Five digits to the right of the decimal for numbers between 0.1 and 999.
In the listing (.lis) file, all .MEASURE output values are in scientific notation
so .OPTION MEASDGT=5 results in five decimal digits.
See Also
.OPTION INGOLD
.MEASURE (or) .MEAS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
539
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MEASFAIL
.OPTION MEASFAIL
Specifies where to print the failed measurement output.
Syntax
.OPTION MEASFAIL=0|1
Default
1
Description
Use this option to specify where to print the failed measurement output. You
can assign this option the following values:
■
MEASFAIL=0, outputs “0” into the .mt#, .ms#, or .ma# file, and prints “failed”
in the .lis file.
■
MEASFAIL=1, prints “failed” in the .mt#, .ms#, or .ma# file, and in the .lis
file.
See Also
.MEASURE (or) .MEAS
540
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MEASFILE
.OPTION MEASFILE
Controls whether measure information outputs to single or multiple files when
an .ALTER command is present in the netlist.
Syntax
.OPTION MEASFILE=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to control whether the measure information outputs to a single
or multiple files when an .ALTER command is present in the netlist. You can
assign this option the following values:
■
MEASFILE=0, outputs measure information to several files.
■
MEASFILE=1, outputs measure information to a single file.
See Also
.ALTER
.MEASURE (or) .MEAS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
541
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MEASFORM
.OPTION MEASFORM
Enables writing of measurement output files to Excel or HSIM formats, as well
as the traditional HSPICE *.mt# format.
Syntax
.OPTION MEASFORM=0|1|2|3
Default 0
Description
This option allows specification of file formats other than the traditional HSPICE
*mt#, *ms#, and *ma# measure output files to include Excel or HSIM file
formats.
■
0: Writes measure file in traditional default HSPICE output style. (Example
1)
■
1: Writes space-separated style which can be imported as data into Excel
and Microsoft products (requires manual steps in Excel). (Example 2)
■
2: Writes he HSIM style in name=value format. Easy to read, but difficult to
import into standard post-processing tools. (Does not work for *.mc?# files
[see value 3 below] and defaults to HSPICE default output style). (Example
3)
■
3: Writes the comma separated style with suffix *.csv and this format
includes *m?# and *.mc?# files.This style and suffix is understood by
Windows to be an Excel file and can be opened directly in Excel by doubleclicking the file name. (Example 4)
Examples
Results Example 1: Default (Traditional) Measure Format (.option
measform=0)
.TITLE '***inverter circuit***'
delayf
delayr
delay
9.187e-10
5.487e-10
7.337e-10
temper
-25.0000
alter#
1.0000
Results Example 2: Excel Format (.option measform=1)
.TITLE '***inverter circuit***'
delayf
delayr
delay
9.187e-10
5.487e-10
7.337e-10
542
temper
-25.0000
alter#
1.0000
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MEASFORM
Results Example 3: HSIM Format (.option measform=2)
.TITLE '***inverter circuit***'
delayf = 9.187e-10
delayr = 5.487e-10
delay =
7.337e-10
temper =-25.0000
alter# = 1.0000
Results Example 4: CSV-Excel Format (.option measform=3)
*** File name opampmc.ms0_D.csv***
See Also
.OPTION INGOLD
.MEASURE (or) .MEAS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
543
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MEASOUT
.OPTION MEASOUT
Outputs .MEASURE command values and sweep parameters into an ASCII file.
Syntax
.OPTION MEASOUT=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to output .MEASURE command values and sweep parameters
into an ASCII file. Post-analysis processing (WaveView or other analysis tools)
uses this <design>.mt# file, where # increments for each .TEMP or .ALTER
block.
For example, for a parameter sweep of an output load, which measures the
delay, the .mt# file contains data for a delay-versus-fanout plot. You can set this
option to 0 (off) in the hspice.ini file.
See Also
.ALTER
.MEASURE (or) .MEAS
.TEMP (or) .TEMPERATURE
544
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MESSAGE_LIMIT
.OPTION MESSAGE_LIMIT
Limits how many times a certain type warning can appear in the output listing
based on the message index.
Syntax
.OPTION MESSAGE_LIMIT 'message_index:number'
Argument
Description
message_index
Specifies the message index linked below
number
Specifies the limiting number of displays of the message
Description
Use this option to set the number of display times for a certain warning type
based on its message index number.
■
The message_index parameter specifies the message index listed in the
Warning Message Index [10001-10076] or Error Message Index [2000120024], located in the HSPICE User Guide: Simulation and Analysis,
Chapter 34, Warning/Error Messages.
■
The number parameter specifies the display times.
.OPTION MESSAGE_LIMIT has a higher priority than OPTION WARNLIMIT
and increases the coverage of types messages to be limited.
See Also
.OPTION WARNLIMIT (or) .OPTION WARNLIM
.OPTION STRICT_CHECK
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
545
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION METHOD
.OPTION METHOD
Sets the numerical integration method for a transient analysis for HSPICE/
HSPICE RF.
Syntax
.OPTION METHOD=GEAR | TRAP [PURETP] | BDF
Default
TRAP
Description
Use this option to set the numerical integration method for a transient analysis.
■
TRAP selects trapezoidal rule integration. This method inserts occasional
Backward-Euler timesteps to avoid numerical oscillations. You can use the
PURETP option to turn this oscillation damping feature off.
■
TRAP PURETP selects pure trapezoidal rule integration. This method is
recommended for high-Q LC oscillators and crystal oscillators.
■
GEAR selects BDF integration or GEAR integration based on circuit type.
■
GEAR MAXORD=2|3 selects GEAR integration.
■
GEAR MAXORD=1 prohibits GEAR from selecting BDF.
■
GEAR MU=0 selects Backward-Euler integration.
■
BDF selects the high order integration method based on the backward
differentiation formulation.
Note: To change LVLTIM from 2 to 1 or 3, set LVLTIM=1 or 3 after
the METHOD=GEAR option. This overrides METHOD=GEAR,
which sets LVLTIM=2.
TRAP (trapezoidal) integration usually reduces program execution time with
more accurate results. However, this method can introduce an apparent
oscillation on printed or plotted nodes, which might not result from circuit
behavior. To test this, run a transient analysis by using a small timestep. If
oscillation disappears, the cause is the trapezoidal method.
The GEAR method is a filter, removing oscillations that occur in the trapezoidal
method. Highly non-linear circuits (such as operational amplifiers) can require
very long execution times when you use the GEAR method. Circuits that do not
converge in trapezoidal integration, often converge if you use GEAR.
The BDF method is a high order integration method based on the backward
differentiation formulae. Two tolerance options are available to the user for the
546
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION METHOD
BDF method: .OPTIONS BDFRTOL (relative) and BDFATOL (absolute); each
has a default of 1e-3. BDF can provide a speed enhancement to mixed-signal
circuit simulation, especially for circuits with a large number of devices. The
BDF method currently provides no advantage for use with small circuits in
standard cell characterization. The BDF supported models/devices/elements
and limitations are listed. METHOD=BDF supports the following:
■
Bulk MOSFET, levels 1-54
■
SOI MOSFET, levels 57, 70
■
BJT, levels 1, 2, 3
■
Diodes, all
■
Resistors, all
■
Capacitors (excludes DC block)
■
Independent sources: V and I
■
Dependent sources: E/F/G/H
■
L (excludes AC choke)
■
K (excludes magnetic core, ideal transformer)
■
Signal integrity elements: B (IBIS buffer)/S/ W/ T
Note:
BDF issues a warning in the .lis file if it encounters an
unsupported model. The message is similar to: WARNING!!!,
netlist contains ‘unsupported models’, HSP-BDF
is disabled.
When RUNLVL is turned off (=0), method=GEAR sets bypass=0; the user can
reset bypass value by using .option bypass=value. Also, when RUNLVL
is turned off, there is an order dependency with GEAR and ACCURATE
options; if method=GEAR is set after the ACCURATE option, then the
ACCURATE option does not take effect; if method=GEAR is set before the
ACCURATE option, then both GEAR and ACCURATE take effect.
If GEAR is used with RUNLVL, then GEAR only determines the numeric
integration method; anything else is controlled by RUNLVL; there is no order
dependency with RUNLVL and GEAR. Since there is no order dependency with
RUNLVL and GEAR, or RUNLVL and ACCURATE, then:
is equivalent to
To see how use of the GEAR method impacts the value settings of ACCURATE
and other options, see Appendix B, How Options Affect other Options.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
547
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION METHOD
Examples
Example 1 sets pure trapezoidal method integration. No Gear-2 or BackwardEuler is mixed in. Use this setting when you simulate harmonic oscillators.
Example 1
.option method=trap puretp
Example 2 sets pure Backward-Euler integration.
Example 2
.option method=gear maxord=1
Example 3 sets pure Gear-2 integration.
Example 3
.option method=gear
Example 4 sets the higher order backward differentiation formulation
integration for supported models.
Example 4
.option method=bdf
See Also
.OPTION ACCURATE
.OPTION LVLTIM
.OPTION MAXORD
.OPTION MTTHRESH
.OPTION PURETP
.OPTION MU
.OPTION RUNLVL
.OPTION BDFATOL
.OPTION BDFRTOL
548
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MODMONTE
.OPTION MODMONTE
Controls how random values are assigned to parameters with Monte Carlo
definitions.
Syntax
.OPTION MODMONTE=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Ordinarily, the assignment of a random value is only done once, then used
several times. The exception to this rule is for model parameters. Since a model
definition is only done once, the behavior described above would assign the
same parameter value to all devices referencing that model. To overcome
this, .OPTION MODMONTE lets you decide if all instances of a device should get
the same or unique model parameters. Use this option to control how random
values are assigned to parameters with Monte Carlo definitions.
■
If MODMONTE=1, then within a single simulation run, each device that shares
the same model card and is in the same Monte Carlo index receives a
different random value for parameters that have a Monte Carlo definition.
■
If MODMONTE=0, then within a single simulation run, each device that shares
the same model card and is in the same Monte Carlo index receives the
same random value for its parameters that have a Monte Carlo definition.
Examples
In the following example, transistors M1 through M3 have the same random
vto model parameter for each of the five Monte Carlo runs through the use of
the MODMONTE option.
...
.option MODMONTE=0 $$ MODMONTE defaults to 0;OK to omit this line.
.param vto_par=agauss(0.4, 0.1, 3)
.model mname nmos level=53 vto=vto_par version=3.22
M1 11 21 31 41 mname W=20u L=0.3u
M2 12 22 32 42 mname W=20u L=0.3u
M3 13 23 33 43 mname W=20u L=0.3u
...
.dc v1 0 vdd 0.1 sweep monte=5
.end
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
549
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MODMONTE
In Example 2, transistors M1 through M3 have different values of the vto
model parameter for each of the Monte Carlo runs by the means of setting
.option MODMONTE=1.
Example 1
...
.option MODMONTE=1
.param vto_par=agauss(0.4, 0.1, 3)
.model mname nmos level=54 vto=vto_par
M1 11 21 31 41 mname W=20u L=0.3u
M2 12 22 32 42 mname W=20u L=0.3u
M3 13 23 33 43 mname W=20u L=0.3u
...
.dc v1 0 vdd 0.1 sweep monte=5
.end
See Also
.MODEL
550
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MODPRT
.OPTION MODPRT
Invokes model-preprocressing and parameter flattening.
Syntax
.OPTION MODPRT=[0|1]
Default 0 (Off)
Description
When .OPTION MODPRT=1 the following takes place:
■
Model information is written to a file called reduced.models, readable by
standard HSPICE.
■
Information for each model occupies a single physical record to facilitate
further processing necessary to link the new models to the cell library.
■
Comments can appear between the model records (to help tracing).
■
Values are printed to 17 digits to simplify validation.
■
Fields that are missing on the original model record are not be printed (to
avoid warnings and potential errors in HSPICE).
■
Fields for which the values equal the default values for the particular level/
version are not printed, thus reducing the size of the file; all other fields
appearing on the original model card are printed.
■
Since each MOSFET has its own model in the reduced.models file, the bin
designator is replaced by the index of the MOSFET. For example, a model
name is pch_27 because the device belongs to bin 27.
■
Since the models are non-binned, the extra fields: lmin, lmax, wmin, wmax
(and similar fields, if any), are deleted.
■
A reduced.instances file is generated in cases where additional information
is required for the instance. For example, for the “main n1 …" call inside the
subckt, the parameters on the MOSFET need not be the same as what were
specified on the subckt invocation. The reduced.instances file reports the
MOSFET records with the resolved values for the parameters.
See the examples below for additional information.
Examples
Example 1
Original Netlist: In the case below, it is assumed that:
(1) X_1 and X_2 use the same bin model card pch.26, while there are
some different parameters values in model cards (because instance
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
551
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MODPRT
X_1
X_2
X_3
X_4
X_5
1
1
1
1
1
Example 2
.model
.model
.model
Example 3
X_1
X_2
X_3
X_4
X_5
parameters will affect the model parameters values);
(2) X_3 and X_4 could share the model card with X_1;
(3) X_5 could not share model card with other instance, and it uses the
pch_4 model card;
2 0 0
pch_mac
W=… L=…
2 0 0
nch_mac
W=… L=…
2 0 0
pch_mac
W=… L=…
2 0 0
nch_mac
W=… L=…
2 0 0
pch_mac
W=… L=…
reduced.models output file for Example 1: This file prints unique model
cards and adds instance name information on model card name.
X_1_pch_26
level = 54 ……
X_2_pch_26
level = 54 ……
X_5_pch_4
level = 54 …..
reduced.instance file: this file connects the model information with
instance information as shown below.
X_1_pch_26
W = …… L = ……
X_2_pch_26
W = …… L = ……
X_1_pch_26
W = …… L = ……
X_1_pch_26
W = …… L = ……
X_5_pch_4
W = …… L = ……
1. In the reduced.instance file, he "." characters by are replaced by "_" in the
model names; a model card name X_1_pch_26 includes two parts:
■
Instance name (X_1)
■
Bin model name (pch_26)
the first part is the instance name (X_1) and the second part is the bin
2. The reduced.instance file does not print the d/g/s/b connecting information;
the format is:
instance name
X_1
model name
X_1_pch_26
solved parameter values
W = …… L = ……
3. The reduced.instance file contains all the fields as they become resolved
inside the macro, not just the ones on the original “X” record.
4. For each model, the information is printed to be a single physical record in
reduced.models (not continued across multiple records with “+” continuation).
552
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MONTECON
.OPTION MONTECON
Continues a Monte Carlo analysis in HSPICE by retrieving the next random
value, even if non-convergence occurs.
Syntax
.OPTION MONTECON=0|1
Default
1
Description
Use this option to retrieve the next random value, even if non-convergence
occurs. A random value can be too large or too small to cause convergence to
fail. Other types of analyses can use this Monte Carlo random value.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
553
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MOSRALIFE
.OPTION MOSRALIFE
Invokes the MOSRA “lifetime” computation.
Syntax
.OPTION MOSRALIFE=degradation_type_keyword
Description
Use this option to compute device lifetime calculation for the degradation type
specified.
The option is used in conjunction with .OPTION DegF=valwhen no values are
set for either .OPTION DegFN=val or .OPTION DegFP=val, the designated
NMOS's or PMOS’s failure criteria for lifetime computation, respectively. The
options apply to all MOSFETs. The lifetime value is printed in the RADEG file.
See Also
.OPTION DEGF
.OPTION DEGFN
.OPTION DEGFP
.OPTION RADEGFILE
.OPTION RADEGOUTPUT
554
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MOSRASORT
.OPTION MOSRASORT
Enables the descending sort for reliability degradation (RADEG) output.
Syntax
.OPTION MOSRASORT=degradation_type_keyword
Default delvth0
Description
Use this option mosrasort to enable the descending sort for reliability
degradation (RADEG) output.
If the mosrasort option is not specified, or the degradation type keyword is
not recognized, HSPICE does not do the sorting. (Degradation type keywords
are listed in the HSPICE Application Note: Unified Custom Reliability Modeling
API (MOSRA API), available by contacting the HSPICE technical support
team.)
If you only specify the option mosrasort, and do not specify the degradation
type keyword, HSPICE sorts RADEG by the delvth0 keyword.
HSPICE sorts the output in two separate lists, one for NMOS devices, another
for PMOS device. HSPICE prints the NMOS device list first, and then the
PMOS device list.
Examples
In the following usage, the option does a descending sort for RADEG output on
delvth0’s value.
.option mosrasort=delvth0
See Also
.MOSRA
MOSFET Model Reliability Analysis (MOSRA)
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
555
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MRAAPI
.OPTION MRAAPI
Loads and links the dynamically linked MOSRA API library.
Syntax
.OPTION MRAAPI=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to load and link the compiled MOSRA API .so library file to
HSPICE during simulation. If this option parameter is set with no value or to 1,
then the MOSRA API .so library file is loaded as a dynamically-linked object
file.
If this option parameter does not exist in the netlist, or is explicitly set to 0, the
MOSRA API .so library will not be used.
556
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MRAEXT
.OPTION MRAEXT
Enables access to MOSRA API extension functions.
Syntax
.OPTION MRAEXT 0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to control the access to the MOSRAAPI extension functions.
When MRAEXT=1, HSPICE can access the extension functions. Details are in
the HSPICE User Guide: Implementing the MOSRA API. Contact HSPICE
Technical Support for more information.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
557
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MRAPAGED
.OPTION MRAPAGED
Enables the MOSRA API to enable two modes of model parameter
degradation.
Syntax
.OPTION MRAPAGED=0|1
Default
0
Description
If this option parameter does not exist (deemed as default) in the netlist, or is
explicitly set to 0, degradation from the MOSRA API model is the parameter
value shift with regard to the fresh model, delta_P. If this option parameter is set
to 1, then the degradation from the MOSRA API model is the degraded model
parameter, P+delta_P.
558
■
0: delta_P mode
■
1: Degraded model parameter
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MRA00PATH, MRA01PATH, MRA02PATH, MRA03PATH
.OPTION MRA00PATH, MRA01PATH, MRA02PATH,
MRA03PATH
These options support file path access in MOSRA API functions.
Syntax
.OPTION MRA00PATH ='file_path1'
.option MRA01PATH ='file_path2'
.option MRA02PATH ='file_path3'
.option MRA03PATH ='file_path4'
Default NULL for each path
Description
Use these options to enable global string type variables such as user-defined
paths. This option is for API model developers to access the MOSRA API
functions.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
559
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MTTHRESH
.OPTION MTTHRESH
Reduces the default active device limit for multithreading.
Syntax
.OPTION MTTHRESH=N
Default
64
Description
Use .OPTION MTTHRESH only for model evaluation threading. For
multithreading to be effective in model evaluation, the number of active devices
or elements should meet certain requirements.
The condition for model evaluation to be multithreaded is ONE of the following:
■
MOSFET >= 64
■
BJT >= 128
■
Diode >= 128
■
G-element >= 128
■
E-element >= 128
■
F-element >= 128
■
H-element >= 128
■
or parameter expressions >= 64
If the circuit lacks the required number of active devices, HSPICE automatically
uses a single thread. You can manually enforce multithreading on model
evaluation by using .OPTION MTTHRESH. The default MTTHRESH value is 64.
You can set it to any positive integer number equal to or greater than 2. This
option has no effect on matrix solving. MTTHRESH must = 2 or more. Otherwise,
HSPICE MT defaults to 64.
Examples
If MTTHRESH=50, model evaluation of MOSFETs would be threaded if the
number of MOSFETs is greater than 50. Similarly, a diode model evaluation
would receive benefit from multithreading if the circuit contains more than 100
(50 x 2) diodes.
560
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION MU
.OPTION MU
Defines the integration method coefficient.
Syntax
.OPTION MU=x
Default
0.5
Description
Use this option to define the integration method coefficient. The value range is
0.0 to 0.5. The default integration method is trapezoidal which corresponds to
the default coefficient value of 0.5. If the value is set to 0, then the integration
method becomes backward-Euler. A value between 0 and 0.5 is a blend of the
trapezoidal and backward-Euler integration methods.
See Also
.OPTION METHOD
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
561
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NCFILTER
.OPTION NCFILTER
Filters negative conductance warning messages according to the setting value.
Syntax
.OPTION NCFILTER=val
Default –1e–12
Description
When .option ncwarn is set, use this option to filter the negative
conductance warning messages according to the setting value. If gds, gm,
gmbs < value, a warning message is reported. When ncwarn is set, this filter is
automatically enabled. The legal range of val is –1e20 to 0.
See Also
.OPTION NCWARN
562
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NCWARN
.OPTION NCWARN
Allows turning on a switch to report a warning message for negative
conductance on MOSFETs.
Syntax
.OPTION NCWARN=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use the option to turn on (.option NCWARN=1), printing out of the first
occurrence of MOSFET related “negative conductance” in the listing file; if you
want to check the entire negative conductance on MOSFETs, use.option
DIAGNOSTIC to print all these warning messages.NCWARN=0 (default) turns off
all warning messages on negative conductance.
See Also
.OPTION DIAGNOSTIC (or) .OPTION DIAGNO
.OPTION NCFILTER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
563
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NEWTOL
.OPTION NEWTOL
Calculates one or more iterations past convergence for every calculated DC
solution and timepoint circuit solution.
Syntax
.OPTION NEWTOL=x
Description
Use this option to calculate one or more iterations past convergence for every
calculated DC solution and timepoint circuit solution. If you do not set NEWTOL
after HSPICE determines convergence the convergence routine ends and the
next program step begins.
564
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NODE
.OPTION NODE
Prints a node cross-reference table.
Syntax
.OPTION NODE=x
Description
Use this option to print a node cross-reference table. The BRIEF option
suppresses NODE. The table lists each node and all elements connected to it. A
code indicates the terminal of each element. A colon (:) separates the code
from the element name.
The codes are:
+ — Diode anode
- — Diode cathode
B — BJT base
B — MOSFET or JFET bulk
C — BJT collector
D — MOSFET or JFET drain
E — BJT emitter
G — MOSFET or JFET gate
S — BJT substrate
S — MOSFET or JFET source
Examples
This sample part of a cross-reference line indicates that the bulk of M1, the
anode of D2 and the base of Q4, all connect to node 1.
See Also
.OPTION BRIEF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
565
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NOELCK
.OPTION NOELCK
Bypasses element checking to reduce preprocessing time for very large files.
Syntax
.OPTION NOELCK 0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to bypass element checking to reduce preprocessing time for
very large files. HSPICE typically checks for duplicate element definitions. If
.option NOELCK is set (1), HSPICE skips the element checking and the
simulation runs even if there is a duplicate element definition. For the duplicate
elements, HSPICE uses the last definition it finds.
When NOELCHK is not turned on, if HSPICE finds a duplicate element
definition, it issues an error and aborts the simulation.
Note:
Subcircuit redefinition is not supported by this option.
Examples
In the following netlist:
R1
R2
C1
C1
1
2
2
2
2 1k
0 1k
end 1p
0 1n
...unless .option NOELCHK is set to 1, HSPICE aborts the simulation and
issue an error message.
**error** attempts to redefine c1 at line xx and line yy
566
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NOISEMINFREQ
.OPTION NOISEMINFREQ
Specifies the minimum frequency of noise analysis in HSPICE/HSPICE RF.
Syntax
.OPTION NOISEMINFREQ=x
Description
Use this option to specify the minimum frequency of noise analysis. If the
frequency of noise analysis is smaller than the minimum frequency, then
HSPICE automatically sets the frequency for NOISEMINFREQ.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
567
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NOMOD
.OPTION NOMOD
Suppresses the printout of model parameters.
Syntax
.OPTION NOMOD=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to suppress the printout of model parameters.
568
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NOPIV
.OPTION NOPIV
Controls whether HSPICE automatically switches to pivoting matrix factors.
Syntax
.OPTION NOPIV=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to prevent HSPICE from automatically switching to pivoting
matrix factors if a nodal conductance is less than PIVTOL. NOPIV=1 inhibits
pivoting.
See Also
.OPTION PIVTOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
569
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NOTOP
.OPTION NOTOP
Suppresses topology checks to increase preprocessing speed.
Syntax
.OPTION NOTOP=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to suppress topology checks to increase the speed for
preprocessing very large files. HSPICE normally checks the netlist topology
and reports a warning or error message. The different topologies that HSPICE
checks includes inductor/voltage loops, dangling nodes, stacked current
sources and current sources in a closed capacitor loop. If you set the NOTOP
option to 1, these checks will not be performed and there will be no warning or
error messages issued for these topologies.
Examples
If you run the following netlist:
R1 1 2 1k
R2 2 0 1k
C1 2 end 1p
...the dangling node check function causes HSPICE to issue a warning in
the .lis file.
only 1 connection at node 0:end ...
If .option NOTOP is set, the topology check is skipped and you will not get
the warning.
570
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NOWARN
.OPTION NOWARN
Suppresses parameter conflict warning messages.
Syntax
.OPTION NOWARN=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to suppress all conflicting parameter warning messages, except
those generated from commands in .ALTER blocks.
.OPTION WARNLIMIT can be used to limit the number of a same warning
message.
Note:
This option only suppresses warnings about conflicting
parameters, not model-related or other warnings.
See Also
.ALTER
.OPTION WARNLIMIT (or) .OPTION WARNLIM
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
571
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NUMDGT
.OPTION NUMDGT
Controls the listing printout accuracy.
Syntax
.OPTION NUMDGT=x
Description
Use this option to control the listing printout (.lis) accuracy. The value of x is
typically between 1 and 7, although you can set it as high as 10. This option
does not affect the accuracy of the simulation.This option does, however, affect
the results files (ASCII and binary) if you use the
.OPTIONPOST_VERSION=2001 setting. The default setting is 5 digits for
results for printout accuracy when using POST_VERSION=2001.
See Also
.OPTION POST_VERSION
572
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NUMERICAL_DERIVATIVES
.OPTION NUMERICAL_DERIVATIVES
Diagnostic-only option for checking a problem with the device models.
Syntax
.OPTION NUMERICAL_DERIVATIVES=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
This option can be used to help diagnose convergence problems or suspected
inaccuracies in small-signal analyses such as HBAC, HBNOISE, or
PHASENOISE. If a convergence or accuracy problem stems from an
inaccuracy in the current or charge derivatives returned by a transistor or diode
model, setting this option to 1 will resolve the problem, although with a
performance decrease.
If NUMERICAL_DERIVATIVES=1 resolves the problem, please contact
Synopsys support so that the underlying transistor model issue can be
resolved.
If you are confident that the models are providing accurate derivatives, do not
use this option.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
573
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION NXX
.OPTION NXX
Stops echoing (printback) of the data file to stdout.
Syntax
.OPTION NXX=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to terminate echoing (printback) of the data file to stdout until
HSPICE finds an .OPTION BRIEF=0 or the .END command. It also resets
the LIST, NODE and OPTS options and sets NOMOD. When BRIEF=0, it enables
printback.NXX is the same as BRIEF.
See Also
.OPTION BRIEF
.OPTION LIST
.OPTION NODE
.OPTION OPTS
574
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OFF
.OPTION OFF
Initializes terminal voltages to zero for active devices not initialized to other
values.
Syntax
.OPTION OFF=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to initialize terminal voltages to zero if you did not initialize them
to other values for all active devices. For example, if you did not initialize both
drain and source nodes of a transistor (using .NODESET, .IC commands, or
connecting them to sources), then OFF initializes all nodes of the transistor to 0.
HSPICE checks the OFF option before element IC parameters. If you assigned
an element IC parameter to a node, simulation initializes the node to the
element IC parameter value, even if the OFF option previously set it to 0.
You can use the OFF element parameter to initialize terminal voltages to 0 for
specific active devices. Use the OFF option to help find exact DC operatingpoint solutions for large circuits.
See Also
.DC
.IC
.NODESET
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
575
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OPFILE
.OPTION OPFILE
Outputs the operating point information to a file.
Syntax
.OPTION OPFILE=[0|1|2]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to output the operating point information to a file. When back
annotating the operating point information for the Synopsys Galaxy Custom
Designer product, use this option =1 in conjunction with .OPTION
SPLIT_DP=1.
■
0: The operating point information outputs to stdout.
■
1: The operating point information is output to a file named design.dp#.
■
2: The operating point information is output to multiple separate *.dp# files.
When used with multiprocessing (-mp) .OPTION OPFILE=1 or 2 is valid (3 is
ignored).
See Also
.OP
.OPTION SPLIT_DP
576
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OPTCON
.OPTION OPTCON
Continues running a bisection analysis (with multiple .ALTER commands) even
if optimization failed.
Syntax
.OPTION OPTCON=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to override how HSPICE treats bisection measure failure. With
this option turned on, Instead of issuing an error and exiting the simulation,
HSPICE treats a bisection search failure like a measurement failure and
completes the simulation, or continues if .ALTER commands are specified.
Examples
.option optcon=1
r1 1 0 2000
v1 1 0 3
.param target=0.5
.param x=opt1(0, 0, 1)
.model opt_model opt method=bisection relout=1e6
relin=0.0005
.meas tran y param = x goal = target
.tran 1.0e-10 1.0e-9 sweep optimize=opt1 results=y
model=opt_model
.alter target=1.5
.param target=1.5
.alter target=0.75
.param target=0.75
.end
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
577
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OPTCON
If a bisection search fails because of endpoints having the same sign, for
example, screen output might appear as follows:
>info: ***** hspice job concluded
the maximum number of iterations ( 14)was
exceeded. however, results might be accurate.
x = 3.556e-09
y = 1.7103E+00
>info: ***** hspice job concluded
**Warning** endpoints have same sign in bisection
x = failed
y = failed
>info: ***** hspice job concluded
Output stored in file => test.lis
See Also
.ALTER
.OPTION MEASFAIL
578
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OPTLST
.OPTION OPTLST
Outputs additional optimization information.
Syntax
.OPTION OPTLST=0|1|2|3
Default 0
Description
Use this option to output additional optimization information:
■
OPTLST=0: No information (default).
■
OPTLST=1: Prints parameter, Broyden update and bisection results
information.
■
OPTLST=2: Prints gradient, error, Hessian, and iteration information.
■
OPTLST=3: Prints all of the above and Jacobian.
Since the results of each iteration during an optimization do not meet the
defined electrical specifications, HSPICE does not allow you to probe the
results at each optimization iteration. However, you can use .OPTION
OPTLST=3 to get the useful information about each iteration.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
579
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OPTPARHIER
.OPTION OPTPARHIER
Specifies scoping rules to options.
Syntax
.OPTION OPTPARHIER=[GLOBAL|LOCAL]
Description
Use this option to specify scoping rules to options to support local GEOSHRINK
and SCALE options within .SUBCKT commands. As shown in the example
below, when OPTPARHIER=GLOBAL, SCALE=2u GEOSHRINK=0.8 will be valid
in subcircuits.
When OPTPARHIER=LOCAL, SCALE=1e-6 GEOSHRINK=0.9 is valid in
subcircuits.
Examples
This example explicitly shows the difference between local and global scoping
for using options in subcircuits.
.OPTION OPTPARHIER=[global | local]
.OPTION SCALE=2u GEOSHRINK=0.8
.PARAM DefPwid=1u
.SUBCKT Inv a y DefPwid=2u DefNwid=1u
.OPTIONS SCALE=1e-6 GEOSHRINK=0.9
Mp1 MosPinList pMosMod L=1.2u W=DefPwid
Mn1 MosPinList nMosMod L=1.2u W=DefNwid
.ENDS
See Also
.OPTION GEOSHRINK
.OPTION SCALE
.SUBCKT
580
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION OPTS
.OPTION OPTS
Prints current settings for all control options.
Syntax
.OPTION OPTS
Description
Use this option to print the current settings for all control options. If you change
any of the default values of the options, the OPTS option prints the values that
the simulation actually uses. The BRIEF option suppresses OPTS.
Note:
All SIM_LA* printed settings are shown as LA_*.
See Also
.OPTION BRIEF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
581
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PARHIER (or) .OPTION PARHIE
.OPTION PARHIER (or) .OPTION PARHIE
Specifies scoping rules.
Syntax
.OPTION PARHIER=[GLOBAL|LOCAL]
Description
Use this option to specify scoping rules. The example explicitly shows the
difference between local and global scoping for using parameters in subcircuits.
Examples
.OPTION parhier=global | local
.PARAM DefPwid=1u
.SUBCKT Inv a y DefPwid=2u DefNwid=1u
Mp1 <MosPinList> pMosMod L=1.2u W=DefPwid
Mn1 <MosPinList> nMosMod L=1.2u W=DefNwid
.ENDS
582
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PATHNUM
.OPTION PATHNUM
Prints subcircuit path numbers instead of path names; overrides 8-character
model name limitation.
Syntax
.OPTION PATHNUM=[0|1|2]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
When set to 1, this option prints subcircuit path numbers instead of path
names. When set to 2, the complete model name (no truncation) is printed to
the *.lis file; without this setting, model names are limited to eight characters. In
addition, a full nodal hierarchy table is printed. For example, the following
captab nodal hierarchy appears as:
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
583
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PCB_SCALE_FORMAT
.OPTION PCB_SCALE_FORMAT
Extends support for using a scaling factor in place of the decimal point for PCB
part number formats during case-sensitive simulation.
Syntax
.OPTION PCB_SCALE_FORMAT=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Allows both uppercase and lowercase number formats to be supported when
case sensitive simulations are run for parts places on a PCB. This option
maintains backward compatibility for those who use a number format that is
common for parts placed on a PCB, where the scaling factor is used instead of
the decimal point (e.g., 3k3 -> 3.3k).
Setting .OPTION PCB_SCALE_FORMAT= 1 when case-sensitivity is turned on
allows the 3k3 number format to be usable in an expression.
This option adds a new scaling factor, “r” or “R,” which is the multiplying factor
1e0 (often used for resistors).
Examples
Example 1
Decimal converted to Expression
.option pcb_scale_format=1
.param a='3k3 +2k/2'
As seen in the examples below, backward compatibility with the features of
HSPICE numbers is maintained (such as optional trailing units and scaling
symbols). The examples below show how the values 0 or 1 affect the output.
Example 2
.OPTION PCB_SCALE_FORMAT=0:
1) 0u1 / 0U1 / 0u1farads / 0.1u / 0u1farads / 0.1ufarads -> 0.1u
2) 5R6 / 5r6 / 5600m0 / 5600M0 / 5600m -> 5.6
3) 5MEG35 / 5meg35 / 5.35Meg -> 5.35e6
Example 3
.OPTION PCB_SCALE_FORMAT=1:
a) 0u1 / 0u1farads / 0.1u -> 0.1u
b) 5R6 / 5r6 / 5600m0 / 0M0000056-> 5.6
c) 5MEG35 / 5meg35 -> 5.35e6
584
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PCB_SCALE_FORMAT
See Also
.OPTION SI_SCALE_SYMBOLS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
585
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHASENOISEKRYLOVDIM
.OPTION PHASENOISEKRYLOVDIM
Specifies the dimension of the Krylov subspace that the Krylov solver uses.
Syntax
.OPTION PHASENOISEKRYLOVDIM
Default
500
Description
Specifies the dimension of the Krylov subspace that the Krylov solver uses.
This must be an integer greater than zero.
See Also
.OPTION BPNMATCHTOL
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER
.OPTION PHASENOISETOL
.OPTION PHNOISELORENTZ
586
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER
.OPTION PHASENOISEKRYLOVITER (or)
PHASENOISE_KRYLOV_ITER
Specifies the maximum number of Krylov iterations that the phase noise Krylov
solver takes.
Syntax
.OPTION PHASENOISEKRYLOVITER | PHASENOISE_KRYLOV_ITER
Default
1000
Description
Specifies the maximum number of Krylov iterations that the phase noise Krylov
solver takes. Analysis stops when the number of iterations reaches this value.
See Also
.OPTION BPNMATCHTOL
.OPTION PHASENOISEKRYLOVDIM
.OPTION PHASENOISETOL
.OPTION PHNOISELORENTZ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
587
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHASENOISETOL
.OPTION PHASENOISETOL
Specifies the error tolerance for the phase noise solver.
Syntax
.OPTION PHASENOISETOL
Default
1e-8
Description
Specifies the error tolerance for the phase noise solver. This must be a real
number greater than zero.
See Also
.OPTION BPNMATCHTOL
.OPTION PHASENOISEKRYLOVDIM
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER
.OPTION PHNOISELORENTZ
588
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHASETOLI
.OPTION PHASETOLI
For HB output, aids in reporting when magnitude of phase current is very small.
Syntax
.OPTION PHASETOLI=val
Default 1.e-15
Description
Use this option in a harmonic balance analysis to report the output of the
magnitude of a current phasor as zero. If the current phasor is less than the
PHASETOLI value, then zero phase is reported. (If the magnitude of a current
value is very tiny, the phase does not matter at all.)
See Also
.OPTION PHASETOLV
.HB
.HBAC
.HBLIN
.HBLSP
.HBNOISE
.HBOSC
.HBXF
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
589
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHASETOLV
.OPTION PHASETOLV
For HB output, aids in reporting when magnitude of phase voltage is very small.
Syntax
.OPTION PHASETOLV=val
Default 1.e-15
Description
Use this option in a harmonic balance analysis to report the output of the
magnitude of a voltage phasor as zero. If the voltage phasor is less than the
PHASETOLV value, the phase of that phasor is output as zero. (If the magnitude
of a voltage value is very tiny, the phase does not matter at all.)
See Also
.OPTION PHASETOLI
.HB
.HBAC
.HBLIN
.HBLSP
.HBNOISE
.HBOSC
.HBXF
590
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHD
.OPTION PHD
Facilitates fast OP convergence for BSIM4 testcases.
Syntax
.OPTION PHD=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
When PHD is set to 1 (ON), this option facilitates fast OP convergence for
BSIM4 testcases. The PHD flow may show performance improvement in
simulations that require large DC OP convergence iterations. When PHD is on
but fails to converge, the simulation exits.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
591
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHNOISELORENTZ
.OPTION PHNOISELORENTZ
Turns on a Lorentzian model for the phase noise analysis.
Syntax
.OPTION PHNOISELORENTZ= 0|1|2
Default
1
Description
Turns on a Lorentzian model for the phase noise analysis.
■
0: Uses a linear approximation to a lorentzian model and avoids phasenoise
values >0dB for low offsets
■
1 (default): Applies a lorentzian model to all noise sources
■
2: Applies a lorentzian model to all non-frequency dependent noise sources
See Also
.OPTION BPNMATCHTOL
.OPTION PHASENOISEKRYLOVDIM
.OPTION PHASENOISEKRYLOVITER (or) PHASENOISE_KRYLOV_ITER
.OPTION PHASENOISETOL
592
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PHNOISEAMPM
.OPTION PHNOISEAMPM
Allows you to separate amplitude modulation and phase modulation
components in a phase noise simulation.
Syntax
.OPTION PHNOISEAMPM=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to enable HSPICE RF to calculate separate amplitude (am) and
phase modulation (pm) components using the output and measure syntax of
a .PHASENOISE simulation. A value of 0 sets the Periodic AC (PAC) phase
noise amplitude modulation (AM) component to zero and the results will be
identical to earlier releases. A value of 1 calculates separate AM and phase
noise components. When .OPTION PHNOISEAMPM=1, then
.MEASURE PHASENOISE extends output variables to the set:<am[noise]>
<pm[noise]>
Examples
The following explicitly sets the calculation for separate am and pm calculation.
.opt phnoiseampm=1
See Also
.PHASENOISE
Amplitude Modulation/Phase Modulation Separation
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
593
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PIVOT
.OPTION PIVOT
Selects a pivot algorithm.
Syntax
.OPTION PIVOT=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Set this option to 1 to select a pivot algorithm to achieve convergence in circuits
that produce hard-to-solve matrix equations. PIVOTselects the numerical
pivoting algorithm that is used to manipulate the matrices. Pivoting affects both
DC and transient analysis. Usually the reason for choosing a pivot method
other than the default 0 is that the circuit contains both very large and very
small conductances.
If PIV0T=0, HSPICE automatically changes from a non-pivoting to pivot
strategy if it detects any diagonal-matrix entry less than PIVTOL. This strategy
provides the time and memory advantages of non-pivoting inversion and avoids
unstable simulations and incorrect results. Use .OPTION NOPIV to prevent
HSPICE from pivoting.
The SPARSE option is the same as PIVOT.
See Also
.OPTION NOPIV
.OPTION PIVTOL
594
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PIVTOL
.OPTION PIVTOL
Sets the absolute minimum value for which HSPICE accepts a matrix entry as
a pivot.
Syntax
.OPTION PIVTOL=x
Description
Use this option to set the absolute minimum value for which HSPICE accepts a
matrix entry as a pivot. PIVTOL is used to prevent numeric overflow conditions
like divide by 0. If the conductance is less than the value of PIVTOL, HSPICE
rebuilds the matrix and chooses the PIVOT algorithm. If the conductance is
greater than the value of PIVTOL, the PIVTOL value replaces the conductance
in the matrix. When a non-pivot algorithm is selected by setting PIVOT=0, then
pivtol is the minimum conductance in the matrix and not a pivot.
The default value of PIVTOL is 1e-15 and the range of PIVTOL is Min:1e-35,
Max:1, excluding 0. The value of PIVTOL must be less than GMIN or GMINDC.
Values that approach 1 increase the pivot. The example below shows how you
can correct a “maximum conductance on node error.”
Note:
If PIVTOL is set too small, you run the risk of creating an overflow
condition and a convergence problem. If you set the value to 0,
an out-of-bounds error is reported.
Examples
If you get an error message such as:
**error** maximum conductance on node 1:v75 } =( 9.2414D-23) is
less than pivtol in transient analysis.
Check hookup for this node, set smaller option pivtol and rerun.
—the error message informs that the node conductance value is less than the
value of PIVTOL. Decrease the PIVTOL value so that it is less than the value in
the error message. The valid range of pivtol values is between 1e-35 to 1,
excluding 0. For this case a setting PIVTOL to 1e-25 resolves the error.
See Also
.OPTION GMIN
.OPTION GMINDC
.OPTION PIVOT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
595
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION POST
.OPTION POST
Saves simulation results for viewing by an interactive waveform viewer.
Syntax
HSPICE Syntax
.OPTION POST=[0|1|2|3|ASCII|BINARY|CSDF]
HSPICE RF Syntax
.OPTION
POST=[0|1|2|3|ASCII|BINARY|CSDF|NW|P|TW|UT|VCD|WDBA]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to save simulation results for viewing by an interactive waveform
viewer and to provide output without specifying other parameters.
Note:
The behavior for .OPTION POST in HSPICE RF is different from
the same option used in HSPICE.
The defaults for the POST option supply usable data to most parameters.
■
POST=0: Does not output simulation results.
■
POST=1, BINARY: (Default if POST is declared without a value) Output
format is binary.
■
POST=2, ASCII: Output format is ASCII.
■
POST=3: Output format is New Wave binary (which enables you to
generate .tr0 files that are larger than 2 gigabytes on Linux platforms).
■
POST=CSDF: Output format is Common Simulation Data Format (Viewlogiccompatible graph data file format).
Options available to HSPICE RF only:
596
■
POST=NW: Output format is XP/AvanWaves.
■
POST=TW: Output format is TurboWave.
■
POST=UT: Output format is Veritools Undertow.
■
POST=VCD: Output format is value change dump. Use with an .LPRINT
command.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION POST
■
POST=WDBA: Output format is XP/CosmosScope.
■
POST=XP: Output format is XP/AvanWaves/CosmosScope.
By default, HSPICE outputs single precision for both time and signal data. If
you want to get double precision data, in the netlist set:
.OPTION POST POST_VERSION=2001
Note:
.OPTION POST in HSPICE is not a global option to dump output
in general and then use other options to specify another format.
Other options such as PSF, CSDF, SDA, ZUKEN override POST if
they are specified after POST, and vice versa. This is unlike
HSPICE RF which allows values beyond
[0|1|2|3|ASCII|BINARY|CSDF].
HSPICE uses the last output control option if multiple output control options are
specified in the netlist.
Examples
In this example the option post overrides the options artist/PSF.
.option artist=2 psf=2
.option post
In this example, the options artist/PSF override the option post.
.option post
.option artist=2 psf=2
See Also
.OPTION POST_VERSION
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
597
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION POSTLVL
.OPTION POSTLVL
Limits the data written to your waveform file to a specified level of nodes.
Syntax
.OPTION POSTLVL=n
Description
Limits the data written to your waveform file to the level of nodes specified by
the n parameter. This option differs from POSTSTOP in that it specifies the
signals of one given level at any level.
Note:
.OPTIONS POSTLVL and POSTTOP are ignored if .OPTION
PROBE is also in the netlist. .OPTION PROBE overrides
POSTLVL and POSTTOP.
Examples
.OPTION POSTLVL=2
This example limits the data written to the waveform file to only the secondlevel nodes (voltage and current).
See Also
.OPTION POSTTOP
.OPTION PROBE
598
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION POST_VERSION
.OPTION POST_VERSION
Specifies the post-processing output version for HSPICE/HSPICE RF.
Syntax
.OPTION POST_VERSION=x
Default 9601
Description
Use this option to set the post-processing output version:
■
x=9007 truncates the node name in the post-processor output file to a
maximum of 16 characters.
■
x=9601 sets the node name length for the output file consistent with input
restrictions (1024 characters) and limits the number of output variables to
9999.
■
x=2001 uses an output file header that displays the correct number of
output variables when the number exceeds 9999. This option also changes
the digit-number precision in results files to match the value of
.OPTIONNUMDGT (when < 5).
By default, HSPICE outputs single precision for both time and signal data. If
you want to get double precision data, in the netlist set:
.OPTION POST POST_VERSION=2001
If you set .OPTION POST_VERSION=2001POST=2 in the netlist, HSPICE
returns more accurate ASCII results.
To use binary values (with double precision) in the output file, include the
following in the input file:
For more accurate simulation results, comment this format.
Examples
If you need to probe more than 9999 signals, set the POST_VERSION option to
2001; for example,
.OPTION POST_VERSION=2001
HSPICE now outputs all the signals into a waveform file and the correct number
of output signals is shown rather than **** when the number of signals exceeds
9999. You can load this waveform file in WaveView to view the signals.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
599
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION POST_VERSION
See Also
.OPTION NUMDGT
.OPTION POST
600
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION POSTTOP
.OPTION POSTTOP
Limits the data written to the waveform file to data from only the top n level
nodes.
Syntax
.OPTION POSTTOP=n
Description
Use this option to limit the data written to your waveform file to data from only
the top n level nodes. This option outputs instances up to n levels deep. If you
do not specify either the PROBE or the POSTTOP options, HSPICE/HSPICE RF
outputs all levels. To enable the waveform display interface, you also need to
specify the .OPTIONPOST option. This option differs from .OPTION POSTLVL
in that it specifies the signals of one or multiple levels from the top level down.
Note:
.OPTIONS POSTTOP and POSTLVL are ignored if .OPTION
PROBE is also in the netlist. .OPTION PROBE overrides
POSTLVL and POSTTOP.
Examples
POSTTOP=3
This example limits the data written to the waveform file to only the three toplevel nodes (voltage and current).
See Also
.OPTION POST
.OPTION PROBE
.OPTION POSTLVL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
601
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PROBE
.OPTION PROBE
Limits post-analysis output to only variables specified in .PROBE and .PRINT
commands for HSPICE/HSPICE RF.
Syntax
.OPTION PROBE=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
When turned on (1), allows you to set post-analysis output to only variables
specified in .PROBE, and PRINT commands. 0=off.By default, HSPICE
outputs all voltages and power supply currents in addition to variables listed
in .PROBE, and .PRINT commands. Using this option can significantly
decrease the sizes of simulation output files.
If .OPTION PROBE is not set:
■
All node voltage and source currents are output to *.tr#, *.ac#, *.sw# files.
■
If measured, the resistor or MOSFET current is also output to *.tr#, *.ac#, or
*.sw# files.
■
If the resistor or MOSFET current are determined by measurement
variables, and .OPTION PUTMEAS is reset (set to 0), these measurement
variables are not output to waveform files.
See Also
.PRINT
.PROBE
.OPTION PROBE
.OPTION PUTMEAS
602
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PSF
.OPTION PSF
In a standalone HSPICE simulation, specifies whether the output is binary
(Parameter Storage Format) or ASCIi. When used with HSPICE RF, specifies
whether binary or ASCII data is output when you run an HSPICE simulation
from the CadenceTM Virtuoso® Analog Design Environment.
Syntax
.OPTION PSF=0|1|2
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to specify whether HSPICE RF outputs binary (Parameter
Storage Format) or ASCII data when you run an HSPICE RF simulation
through the Cadence Virtuoso Analog Design Environment.
If you use .OPTON PSF only (without .OPTION ARTIST), the value of x can be
1 or 2.
■
If .OPTION PSF=1, HSPICE produces binary output.
■
If .OPTION PSF=2, HSPICE produces ASCII output.
When the netlist contains .option psf=2 and a .tran analysis statement
(with no .op statement in the netlist file), HSPICE creates the following output
files:
■
.op0 — dc node voltage and dc operating points
■
.op1 — transient voltage and transient operating points for the transient end
time.
Ordinarily, PSF output is directed to a directory named ./psf to accommodate
the Analog Design Environment. However, HSPICE and Custom Designer
users can redirect PSF output by setting the HSPICE command line option -o
to a directory other than ./psf (for example: -o ../results/input).
Note:
The PSF format is only supported on Sun/SPARC, Red Hat/
SUSE Linux, and IBM AIX platforms, as well as 64-bit versions.
See Also
.OPTION ARTIST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
603
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PURETP
.OPTION PURETP
Specifies the integration method to use for reversal time point in HSPICE/
HSPICE RF.
Syntax
.OPTION PURETP=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to specify the integration method to use for reversal time point.
If you set PURETP=1 and HSPICE finds non-convergence, it uses TRAP
(instead of Bbackward-Euler) for the reversed time point.
Use this option with an .OPTION METHOD=TRAP command to help some
oscillating circuits to oscillate if the default simulation process cannot satisfy the
result.
See Also
.OPTION METHOD
604
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PUTMEAS
.OPTION PUTMEAS
Controls the output variables listed in the .MEASURE command.
Syntax
.OPTION PUTMEAS=0|1
Default
1
Description
Use this option to control the output variables listed in the .MEASURE
command.
■
0: Does not save variable values listed in the .MEASURE command into the
corresponding output file (such as .tr#, .ac# or .sw#). This option decreases
the size of the output file.
■
1: Default. Saves variable values listed in the .MEASURE command to the
corresponding output file (such as .tr#, .ac# or .sw#). This option is similar
to the output of HSPICE 2000.4.
See Also
.MEASURE (or) .MEAS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
605
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PZABS
.OPTION PZABS
Sets absolute tolerances for poles and zeros.
Syntax
.OPTION PZABS=x
Default 1.0e-2
Description
Use this option to set absolute tolerances for poles and zeros in Pole/Zero
analysis. Use this option as follows: If ( X real + X real < PZABS ) , then
X real and X imag = 0 . You can also use this option for convergence tests.
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION LSCAL
.OPTION PZTOL
.OPTION RITOL
606
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION PZTOL
.OPTION PZTOL
Sets the relative tolerance for poles and zeros.
Syntax
.OPTION PZTOL=x
Default
1.0e-6
Description
Use this option to set relative tolerances for poles and zeros in Pole/Zero
analysis.
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION LSCAL
.OPTION PZABS
.OPTION RITOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
607
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RADEGFILE
.OPTION RADEGFILE
Use to specify a MOSRA degradation file name to be used with SIMMODE=1.
Syntax
.OPTION RADEGFILE=file_name
Description
Use this option to specify a MOSRA degradation file name to be used with
SIMMODE=1. HSPICE will read in the degradation information in the specified
file and do a MOSRA post-stress simulation.
Examples
.mosra reltotaltime='10*365*24*60*60' lin=11 simmode=1
.option radegfile = '1.radeg0'
See Also
.MOSRA
.OPTION RADEGOUTPUT
608
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RADEGOUTPUT
.OPTION RADEGOUTPUT
Outputs the MOSRA degradation information to the Word Excel CSV format.
Syntax
.OPTION RADEGOUTPUT=CSV
Description
Use this option to output the MOSRA degradation information to the Microsoft
Excel CSV format. If the CSV value is not specified no CSV file is generated.
See Also
.OPTION RADEGFILE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
609
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RANDGEN
.OPTION RANDGEN
Specifies the random number generator used in traditional Monte Carlo
analysis.
Syntax
.OPTION RANDGEN= [0|‘moa’|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to specify the random number generator used in HSPICE
traditional Monte Carlo analysis. If RANDGEN= ‘moa’ or 1, then a multiplywith-carry type random number generator with longer cycle is used. If
RANDGEN=0, then the traditional random number generator is used.
Note:
The .OPTION SEED command is also valid for the new random
number generator without usage change.
See Also
.OPTION RUNLVL
.OPTION SEED
610
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION REDEFSUB
.OPTION REDEFSUB
Allows redefinition of a subckt in a netlist.
Syntax
.OPTION REDEFSUB =[0|1|2]
Default 0
Description
Enables the redefinition of a subcircuit in a netlist.
■
0: Issues an error message for multiple definitions
■
1: Uses the last declared definition
■
2: Uses the first definition
.option redefsub without a value equals .option redefsub=1.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
611
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELH
.OPTION RELH
Sets the relative current tolerance from iteration to iteration through voltagedefined branches.
Syntax
.OPTION RELH=x
Description
Use this option to set the relative current tolerance through voltage-defined
branches (voltage sources and inductors) from iteration to iteration.
This option can also be used to check current convergence, but only if the value
of the ABSH option is greater than zero.
See Also
.OPTION ABSH
612
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELI
.OPTION RELI
Sets the relative error/tolerance change from iteration to iteration.
Syntax
.OPTION RELI=x
Description
Use this option to set the relative error/tolerance change from iteration to
iteration.
This option determines convergence for all currents in diode, BJT, and JFET
devices. (RELMOS sets tolerance for MOSFETs). This value is the change in
current from the value calculated at the previous timepoint.
■
Default=0.01 for .OPTION KCLTEST=0.
■
Default=1e-6 for .OPTION KCLTEST=1.
See Also
.OPTION RELMOS
.OPTION KCLTEST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
613
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELIN
.OPTION RELIN
(Optimization) Relative input parameter (delta_par_val / MAX(par_val,1e-6)) for
convergence.
Syntax
.OPTION RELIN=value
Default 0.001
Description
(Optimization) Relative input parameter (delta_par_val / MAX(par_val, 1e-6))
for convergence. If all optimizing input parameters vary by no more than RELIN
between iterations, the solution converges. RELIN is a relative variance test so
a value of 0.001 implies that optimizing parameters vary by less than 0.1% from
one iteration to the next. If RELIN is set in .OPTION, the setting of RELIN in the
.model card will be overridden.
Examples
.option RELIN=1e-6 DYNACC
See Also
.MODEL
614
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELMOS
.OPTION RELMOS
Sets the relative error tolerance for drain-to-source current from iteration to
iteration.
Syntax
.OPTION RELMOS=x
Description
Use this option to set the relative error tolerance for drain-to-source current
from iteration to iteration.
This option determines convergence for currents in MOSFET devices while
.OPTION RELI sets the tolerance for other active devices.
This option also sets the change in current from the value calculated at the
previous timepoint. HSPICE uses the .OPTION RELMOS value only if the
current is greater than the .OPTION ABSMOS floor value.
Min value: 1e-07; Max value 10.
See Also
.OPTION ABSMOS
.OPTION RELI
.OPTION RELMOS
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
615
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELQ
.OPTION RELQ
Sets the timestep size from iteration to iteration.
Syntax
.OPTION RELQ=x
Description
Use this option in the timestep algorithm for local truncation error (LVLTIM=2).
If the capacitor charge calculation in the present iteration exceeds that of the
past iteration by a percentage greater than the RELQ value, then HSPICE
reduces the internal timestep (delta). The default is 0.01.
See Also
.OPTION LVLTIM
616
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELTOL
.OPTION RELTOL
Sets the relative error tolerance for voltages from iteration to iteration.
Syntax
.OPTION RELTOL=x
Default
1e-3
Description
Use this option to set the relative error tolerance for voltages from iteration to
iteration. Min value: 1e-20; Max value: 10.
Use this option with the ABSV option to determine voltage convergence.
Increasing x increases the relative error. This option is the same as the RELV
option. The RELI and RELVDC options default to the RELTOL value.
See Also
.OPTION ABSV
.OPTION RELI
.OPTION RELV
.OPTION RELVDC
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
617
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELV
.OPTION RELV
Sets the relative error tolerance for voltages from iteration to iteration.
Syntax
.OPTION RELV=x
Default 1e-3
Description
Use this option to set the relative error tolerance for voltages from iteration to
iteration.
If voltage or current exceeds the absolute tolerances, a RELV test determines
convergence. Increasing x increases the relative error. You should generally
maintain this option at its default value. It conserves simulator charge. For
voltages, this option is the same as the RELTOL option. Min value: 1e-20; Max
value: 10.
See Also
.OPTION RELTOL
618
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELVAR
.OPTION RELVAR
Sets the relative voltage change for LVLTIM=1 or 3 from iteration to iteration.
Syntax
.OPTION RELVAR=x
Description
Use this option to set the relative voltage change for LVLTIM=1 or 3 from
iteration to iteration.
Use this option with the ABSVAR and DVDT timestep algorithm. If the node
voltage at the current timepoint exceeds the node voltage at the previous
timepoint by RELVAR, then HSPICE reduces the timestep and calculates a new
solution at a new timepoint. The default is 0.30, or 30 percent.
For additional information, see “DVDT Dynamic Timestep” in the HSPICE User
Guide: Simulation and Analysis.
See Also
.OPTION ABSVAR
.OPTION DVDT
.OPTION LVLTIM
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
619
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RELVDC
.OPTION RELVDC
Sets the relative error tolerance for voltages from iteration to iteration.
Syntax
.OPTION RELVDC=x
Description
Use this option to set the relative error tolerance for voltages from iteration to
iteration.
If voltages or currents exceed their absolute tolerances, the RELVDC test
determines convergence. Increasing the x parameter value increases the
relative error. You should generally maintain RELVDC at its default value to
conserve simulator charge.
See Also
.OPTION RELTOL
620
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION REPLICATES
.OPTION REPLICATES
Runs replicates of the Latin Hypercube samples.
Syntax
.OPTION REPLICATES=number
Description
When the advanced sampling method Latin Hypercube is used with traditional
Monte Carlo simulation, you can add this option following
.OPTION SAMPLING _METHOD=LHS. This option runs replicates of the Latin
Hypercube samples. The sample with nominal conditions is simulated once.
HSPICE repeats the LHS run the number of times specified by number. For
example, if, in a regular run, you have 10+1 (including nominal value) iterations,
if you set .OPTION REPLICATES=2, you generate 21 (or 2* Value +1) Latin
Hypercube samples.
Examples
.OPTION SAMPLING_METHOD=LHS
.OPTION REPLICATES=2
See Also
.OPTION SAMPLING_METHOD
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
621
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RES_BITS
.OPTION RES_BITS
Tightens tolerances when using HPP (High Performance Parallel) in transient
simulations.
Syntax
.OPTION RES_BITS=n
Default 0
Description
When running a multithread operation in a transient simulation using HPP
(only) this option can be used to tighten convergence tolerances. Tightening
convergence tolerances enable resolving the least significant bit in an n-bit
converter.
Note:
Setting this option may result in increased number of iterations
and, sometimes, slightly increased number of time steps.
Examples
The following example, for a 14-bit A-to-D converter, is set as:
.option res_bits=14
622
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RESMIN
.OPTION RESMIN
Specifies the minimum resistance for all resistors.
Syntax
.OPTION RESMIN=x
Description
Use this option to specify the minimum resistance for all resistors, including
parasitic and inductive resistances. The range is 1e-15 to 10 ohms.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
623
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RISETIME (or) .OPTION RISETI
.OPTION RISETIME (or) .OPTION RISETI
Specifies the smallest signal risetime to be supported in elements and
analyses that are sensitive to frequency bandwidth and time scale constraints.
Syntax
.OPTION RISETIME=x
Default
Calculated automatically (see below)
Description
Use this option to specify the smallest signal risetime to be anticipated when
analyzing certain elements that have frequency dependencies. Several
HSPICE elements require some knowledge regarding either their maximum
frequency of operation, or the minimum signal rise time to be expected. This is
particularly true of elements that are described in the frequency domain, yet
require time-domain simulation. The RISETIME option is used to establish time
scale and frequency scale information needed for inverse Fourier transform
and convolution calculations.
In the W-element (transmission line) model, RISETIME is used to determine
the maximum signal frequency to be taken into account for frequency
dependencies such as skin effect, and dielectric loss (non-zero Rs or Gd).
In the S-element (scattering-parameter) based model, the reciprocal of
RISETIME sets the maximum signal frequency (FMAX) value used for the Sparameter analysis.
In the U-element (lumped transmission line) model, RISETIME is used to set
the number of lumps according to the equation:
TDeff
#lumps = M IN 20, 1 + 20 ⋅ ⎛⎝ ----------------------------⎞⎠
RISETIME
where, TDeff is the end-to-end delay in a transmission line.
When needed, HSPICE automatically calculates a default value for RISETIME
as follows:
624
■
25% of the tstep value specified with the .TRAN command.
■
The time corresponding to a 90-degree phase shift for the highest frequency
specified in SIN, SFFM, and AM sources.
■
The smallest delay time, rise time, fall time, or time increment used in
PULSE, EXP, and PWL sources.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RISETIME (or) .OPTION RISETI
See Also
.MODEL
.OPTION WACC
.OPTION WDELAYOPT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
625
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RITOL
.OPTION RITOL
Sets the minimum ratio value for the (real/imaginary) or (imaginary/real) parts
of the poles or zeros.
Syntax
.OPTION RITOL=x
Default 1.0e-2
Description
Use this option to set the minimum ratio value for the (real/imaginary) or
(imaginary/real) parts of the poles or zeros. Use the RITOL option as follows.
if: X imag ≤ RITOL ⋅ X real , then X imag = 0 . If X real ≤ RITOL ⋅ X imag , then
X real = 0 .
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.PZ
626
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RMAX
.OPTION RMAX
Sets the TSTEP multiplier, which controls the maximum value for the internal
timestep delta fore HSPICE/HSPICE RF.
Syntax
.OPTION RMAX=x
Description
Use this option to set the TSTEP multiplier, which controls the maximum value
(DELMAX) for the delta of the internal timestep:
DELMAX=TSTEP x RMAX
■
The default is 5 if DVDT is 4 and LVLTIM is 1.
■
Otherwise, the default is 2.
Min value: 1e-9; Max value: 1e+9. The RMAX value cannot be smaller than
RMIN.
See Also
.OPTION DELMAX
.OPTION DVDT
.OPTION LVLTIM
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
627
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RMIN
.OPTION RMIN
Sets the minimum value of delta (internal timestep).
Syntax
.OPTION RMIN=x
Description
Use this option to set the minimum value of delta (internal timestep). An
internal timestep smaller than RMIN x TSTEP, terminates the transient analysis,
and reports an internal “timestep too small” error. If the circuit does not
converge in IMAX iterations, delta decreases by the amount you set in the FT
option. The default is 1.0e-9. Min value: 1e-15.
See Also
.OPTION FT
.OPTION IMAX
628
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RUNLVL
.OPTION RUNLVL
Controls runtime speed and simulation accuracy.
Syntax
.OPTION RUNLVL= 1|2|3|4|5|6
Description
Higher values of RUNLVL result in higher accuracy and longer simulation
runtimes; lower values result in lower accuracy and faster simulation runtimes.
For HSPICE:
The RUNLVL option setting controls the scaling of all simulator tolerances
simultaneously, affecting timestep control, transient analysis convergence, and
model bypass tolerances all at once. Higher values of RUNLVL result in smaller
timestep sizes and could result in more Newton-Raphson iterations to meet
stricter error tolerances. RUNLVL settings affect transient analysis only.
RUNLVL can be set to 0 (to disable) 1, 2, 3, 4, 5, or 6:
■
1: Lowest simulation runtime
■
2: More accurate than RUNLVL=1 and faster than RUNLVL=3
■
3: Default value, similar to HSPICE’s original default mode
■
4: More accurate than RUNLVL=3 and faster than RUNLVL=5
■
5 or 6: Corresponds to HSPICE’s standard accurate mode for most circuits:
•
5 is similar to the standard accurate mode in HSPICE
•
6 has the highest accuracy
If RUNLVL is specified in the netlist without a value, the value is the default, 3.
If .OPTION ACCURATE is specified in the netlist together with RUNLVL, the
value of RUNLVL is limited to 5 or 6; specifying a specifying a RUNLVL value of
1, 2, 3, or 4 defaults to 5.
If .OPTION RUNLVL is not turned off, there is no dependency with GEAR and
ACCURATE options, and
.OPTION ACCURATE method=GEAR RUNLVL
is equivalent to
.OPTION method=GEAR ACCURATE RUNLVL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
629
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RUNLVL
The RUNLVL option interacts with other options as follows:
■
Regardless of its position in the netlist, RUNLVL ignores the following step
control-related options (which are replaced by automated algorithms):
LVLTIM DVDT FT FAST TRTOL ABSVARRELVAR RELQ CHGTOL DVTR
IMIN ITL3
■
See the notes to the table below for discussion of options ACCURATE and
BYPASS in relation to RUNLVL if it is specified in the netlist.
■
The tstep value specified with the .TRAN command affects timestep
control when a RUNLVL option is used. Timestep values larger than
tstep*RMAX use a tighter timestep control tolerance.
For information on how RUNLVL values affect other options, see the following
section, and also see RUNLVL=N and RUNLVL, ACCURATE, FAST, GEAR
method in Appendix B of this manual.
For HSPICE RF:
While HSPICE RF supports .OPTION RUNLV, this option is most compatible
with HSPICE. For HSPICE RF, the SIM_ACCURACY option gives you a more
continuous range of settings. You can use .OPTION RUNLVL to control runtime
speed and simulation accuracy. As in HSPICE, higher values of RUNLVL result
in higher accuracy and longer simulations; lower values result in lower
accuracy and faster simulation.
.OPTION RUNLVL maps to .OPTION SIM_ACCURACY as follows:
■
RUNLVL=1: SIM_ACCURACY=0.5
■
RUNLVL=2: SIM_ACCURACY=0.75
■
RUNLVL=3: SIM_ACCURACY=1
■
RUNLVL=4: SIM_ACCURACY=5
■
RUNLVL=5: SIM_ACCURACY=10
■
RUNLVL=6: SIM_ACCURACY=100
Interactions Between .OPTION RUNLVL and Other Options
Since the latest algorithm invoked by RUNLVL sets the timestep and error
tolerance internally, many transient error tolerance and timestep control options
are no longer valid; furthermore, to assure the most efficiency of the new
RUNLVL algorithm, you should let the new engine manage everything itself.
Options that are recommended not to tune are listed in the table, as well.
630
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RUNLVL
Note:
Once RUNLV is set, it does not = 0.
Option
Default value
without RUNLVL
Default value with
RUNLVL=3
User definition
ignored
Recommend
not to tune
ABSV/VNTOL
50u
50u
-
x
ABSVAR
500m
500m
x
-
ACCURATE 1
0
0
-
-
BYPASS a
2
2 for RUNLVL=1-6
-
-
CHGTOL
1.0f
1.0f
x
-
DI
100
100
-
x
DVDT
4
4
x
-
DVTR
1.0k
1.0k
x
-
FAST 2
0
0
x
-
FS
250m
250m
-
x
FT
250m
250m
x
-
IMIN/ITL3
3
3
x
-
LVLTIM
1
4
x
-
METHOD 3
TRAP
TRAP
-
-
RELQ
10m
10m
x
-
RELTOL
1.0m
1.0m
-
x
RELV
1.0m
1.0m
-
x
RELVAR
300.0m
300.0m
x
-
RMAX
5
5
x
-
RMIN
1.0n
1.0n
-
x
TRTOL
7
7
x
-
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
631
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION RUNLVL
1. ACCURATE and BYPASS notes:
1. If .option ACCURATE is set, then the RUNLVL value is limited to 5 or 6. Specifying a RUNLVL less
than 5 results in a simulation at RUNLVL=5. When both ACCURATE and RUNLVL are set, the RUNLVL
algorithm will be used.
2. When RUNLVL is set, BYPASS is set to 2. Users can redefine the BYPASS value by setting .option
BYPASS=value; this behavior is independent of the order of RUNLVL and BYPASS;
2. The FAST option is disabled by the RUNLVL option; setting the RUNLVL value to 1 is comparable
to setting the FAST option.
3. RUNLVL can work with METHOD=GEAR; in cases where GEAR only determines the numeric
integration method during transient analysis, the other options that were previously set by GEAR (when
there is no RUNLVL) now are determined by the RUNLVL mode. This behavior is independent of the
order of RUNLVL and METHOD. See below.
See Also
.OPTION ACCURATE
.OPTION BYPASS
.OPTION DVDT
.OPTION LVLTIM
.OPTION METHOD
.OPTION RELTOL
.TRAN
.OPTION SIM_ACCURACY (RF)
632
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SAMPLING_METHOD
.OPTION SAMPLING_METHOD
Enables use of advanced sampling methods with traditional Gaussian Monte
Carlo trials.
Syntax
.OPTION SAMPLING_METHOD=SRS|LHS|Factorial|OFAT|Sobol|
+ Neiderreiter
Default SRS
Argument
Description
SRS
Simple random sampling performed in traditional HSPICE Monte
Carlo method
LHS
Latin Hypercube sampling; efficient for large number of variable
parameters (used with .OPTION REPLICATES)
Factorial
Factorial sampling;
■
■
Evaluates the circuit response at the extremes of variable ranges
to get an idea of the worst and best case behavior.
Creates polynomial response surface approximations.
OFAT
One-Factor-At-a-Time sampling; useful for sensitivity studies and
for constructing low order response surface approximations.
Sobol
Sobol sampling uses low discrepancy sequences (LDS); LDS
sample points are more frequently distributed compared to LHS and
the sampling error is lower. Sobol is used with a sampling dimension
of 40 or less.
Neiderreiter LDS sampling sequence useful as a sampling method for cases of
a sampling dimension up to 318. If that number is exceeded,
HSPICE switches to the default SRS sampling method.
Description
This option enables use of sampling methods other than Gaussian techniques
available in traditional HSPICE Monte Carlo simulation. For a full discussion
about advanced sampling methods see Comparison of Sampling Methods in
the HSPICE User Guide: Simulation and Analysis. These methods are also
available in the HSPICE Variation Block functionality.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
633
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SAMPLING_METHOD
See Also
.OPTION REPLICATES
634
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SAVEHB
.OPTION SAVEHB
Saves the final-state variable values from an HB simulation.
Syntax
.OPTION SAVEHB=’filename’
Description
Use this option to save the final state (that is, the no-sweep point or the steady
state of the first sweep point) variable values from an HB simulation to the
specified file.
This file can be loaded as the starting point for another simulation by using a
LOADHB option.
See Also
.HB
.OPTION LOADHB
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
635
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SAVESNINIT
.OPTION SAVESNINIT
Saves the operating point at the end of Shooting Newton initialization (sninit).
Syntax
.OPTION SAVESNINIT="filename"
Description
Use this option to save an operating point file at the end of a SN initialization for
use as initial conditions for another Shooting Newton analysis. For more
information, see SN Steady-State Time Domain Analysis in the HSPICE User
Guide: RF Analysis.
See Also
.SN
.OPTION LOADSNINIT
.OPTION SAVESNINIT
.OPTION SNACCURACY
.OPTION SNMAXITER (or) SN_MAXITER
636
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SCALE
.OPTION SCALE
Sets the element scaling factor for HSPICE/HSPICE RF.
Syntax
.OPTION SCALE=x
Description
Use this option to scale geometric element instance parameters whose default
unit is meters. You can also use this option with .OPTION GEOSHRINK to scale
an element even more finely (usually through a technology file). The effective
scaling factor is the product of the two parameters; HSPICE will use
scale*geoshrink to scale the parameters/dimensions.
In HSPICE, the possible geometrical instance parameters include width,
length, or area for both passive and active devices, in addition to the commonly
known MOSFET parameters such as AS, AD, PS, PD, and so on.
■
For active elements, the geometric parameters are:
Diode — W, L, Area JFET/MESFET — W, L, Area MOS — W, L, AS, AD,
PS, PD
■
For passive elements having values calculated as a function geometry, the
geometric parameters are:
Resistor — W, L Capacitor — W, L
In cases where you want to selectively scale a required instance, such as in an
encrypted file, you can use .OPTION HIER_SCALE.
See Also
.OPTION GEOSHRINK
.OPTION BA_SCALE
.OPTION CMIUSRFLAG
.OPTION HIER_SCALE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
637
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SCALM
.OPTION SCALM
Sets the model scaling factor.
Syntax
.OPTION SCALM=x
Description
Use this option to set the scaling factor defined in a .MODEL command for an
element. See the HSPICE Elements and Device Models Manual for parameters
that this option scales. For MOSFET devices, this option is ignored in Level 49
and higher model levels. See the HSPICE Reference Manual: MOSFET
Models for levels available to the SCALM option.
See Also
.MODEL
638
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SEARCH
.OPTION SEARCH
Automatically accesses a library or individual vendor files.
Syntax
.OPTION SEARCH=‘directory_path’ [path_name]
Description
Use this option to auto-access a library, or, using path_name, to search for
library (*.lib) files. Typically, vendors supply part files containing a single
subcircuit. The name of the file is the same as the subcircuit with the file
extension *.inc. The commands .LIB.INC, and .LOAD search for the file. In
addition, HSPICE supports .OPTION SEARCH for .VEC commands. The path
can be given as '/remote/home1/aa' or as '../'
Examples
.OPTION SEARCH=‘$installdir/parts/vendor’
This example searches for models in the vendor subdirectory, under the
$installdir/parts installation directory (see Figure 14). The parts
directory contains the DDL subdirectories.
x1 in out vdd vss buffer_f
.OPTION search=’$installdir/parts/vendor’
$installdir/parts/vendor/buffer_f.inc
$installdir/parts/vendor/skew.dat
.lib ff $ fast model
.param vendor_xl=-.1u
.inc ‘$installdir/parts/vendor/model.dat’
.endl ff
.macro buffer_f in out vdd vss
.lib ‘$installdir/parts/vendor/skew.dat’ ff
.inc ‘$installdir/parts/vendor/buffer.inc’
.eom
$installdir/parts/vendor/buffer.inc
$installdir/parts/vendor/model.dat
.macro buffer in out vdd vss
m1 out in vdd vdd nch w=10 l=1
...
.model nch nmos level=28
+ xl=vendor_xl ...
Note: The ‘/usr’ directory is in the HSPICE install directory.
Figure 14
Vendor Library Usage
See Also
Signal Integrity Examples for netlists using .OPTION SEARCH including
iotran.sp, qa8.sp, and qabounce.sp.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
639
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SEED
.OPTION SEED
Specifies the starting seed for the random-number generator in Monte Carlo
analysis.
Syntax
.OPTION SEED=x | ‘random’
Description
Use this option to specify the starting seed for the random-number generator in
HSPICE Monte Carlo analysis. The minimum value is 1; the maximum value of
is 259200 of SEED. If SEED='random', HSPICE assigns a random number
between 1 and 259200 according to the system clock and prints it in the .lis file
for you to debug. .OPTION SEED is supported In HSPICE and the RF flow.
See Also
.OPTION RANDGEN
640
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SHRINK
.OPTION SHRINK
Scales the final constant capacitance value (only works with .OPTION
CMIUSRFLAG=3).
Syntax
.OPTION SHRINK= val
Description
Use this option to scale the final constant capacitance value. The default
setting overrides .OPTION SHRINK before applying shrink*shrink scaling
to constant capacitance value. The following is the usage of .OPTION SHRINK
and instance parameter shrink:
■
1: If both .OPTION SHRINK and the shrink instance are not set in the
netlist, do nothing.
■
2: If only .OPTION SHRINK is set in the netlist, use it to scale the final
constant capacitance value.
■
3: If the instance parameter shrink is set in the netlist, use the instance
shrink to scale the final constant capacitance value.
See Also
.OPTION CMIUSRFLAG
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
641
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_ACCURACY
.OPTION SIM_ACCURACY
Sets and modifies the size of timesteps.
Syntax
.OPTION SIM_ACCURACY=value
Default
Conditional, see below
Description
Use this option to set and modify the size of timesteps. This option applies to all
modes and tightens all tolerances, such as: Newton-Raphson tolerance, local
truncation error, and other errors.
The value must be a positive number. The default is 1. If you specify .OPTION
ACCURATE, the default value is 10; you can use .option sim_accuracy=10
instead of .option accurate. They are interchangeable. You can set
.option sim_accuracy=10 if you have not set previous sim_accuracy
settings that are 10 or greater or have previously set .option accurate.
To set global accuracy, use .OPTION SIM_ACCURACY=n, where n is a
number greater than 0.
You can apply different accuracy settings to different blocks or time intervals.
The syntax to set accuracy on a block, instance, or time interval is similar to the
settings used for a power supply.
Examples
This example sets accuracy to 3 for the XNAND1 and XNAND2 instances and
4 for all instances of the INV subcircuit. Globally, the accuracy is 2. If accuracy
settings conflict, then HSPICE RF uses the higher accuracy value. At 12.0ns
before the end of the simulation, the global accuracy level is 5. Because this is
higher than 2, 3, or 4, it overrides all previous settings.
.OPTION
.OPTION
.OPTION
.OPTION
.OPTION
.OPTION
.OPTION
SIM_ACCURACY=2
SIM_ACCURACY=3
SIM_ACCURACY=4
SIM_ACCURACY=5
SIM_ACCURACY=5
SIM_ACCURACY=3
SIM_ACCURACY=5
|
|
|
|
|
|
XNAND1 XNAND2
@INV
12.0n
20n
40ns
20ns 3 | 35ns 7 | 50ns
See Also
.OPTION FFT_ACCURATE
.OPTION ACCURATE
642
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DELTAI
.OPTION SIM_DELTAI
Sets the selection criteria for current waveforms in WDB and NW format.
Syntax
.OPTION SIM_DELTAI=value
Default
0 amps
Description
Use this option to set the selection criteria for RF current waveforms in WDB
and NW format (see “Eliminating Current Datapoints” in the HSPICE User
Guide: RF Analysis).The value parameter specifies the amount of change.
Examples
In this example, at the n timestep, HSPICE RF saves only data points that
change by more than 0 amps from previous values at the n-1 timestep.
.OPTION SIM_DELTAI = 0amps
See Also
.OPTION SIM_DELTAV
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
643
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DELTAV
.OPTION SIM_DELTAV
Sets the selection criteria for current waveforms in WDB and NW format.
Syntax
.OPTION SIM_DELTAV=value
Default
1mv
Description
Sets the selection criteria for RF current waveforms in WDB and NW format
(see “Eliminating Voltage Datapoints” in the HSPICE User Guide: RF Analysis).
The value parameter specifies the amount of change.
Examples
In this example, at the n timestep, HSPICE RF saves only data points that
change by more than 1 mV from their previous values at the n-1 timestep.
.OPTION SIM_DELTAV = 1mv
See Also
.OPTION SIM_DELTAI
644
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF
.OPTION SIM_DSPF
Runs simulation with standard DSPF expansion of all nets from one or more
DSPF files.
Syntax
.OPTION SIM_DSPF=“[scope] dspf_filename”
Description
Use this option to run simulation with standard DSPF expansion of all nets from
one or more DSPF files.
scope can be a subcircuit definition or an instance. If you do not specify
scope, it defaults to the top-level definition.
You can repeat this option to include more DSPF files.
This option can accelerate simulation by more than 100%. You can further
reduce total CPU time by including the .OPTION SIM_LA in the netlist.
For designs of 5K transistors or more, including .OPTION SIM_DSPF_ACTIVE
in your netlist to expand only active nodes also provides a performance gain.
Note:
HSPICE RF requires both a DSPF file and an ideal extracted
netlist. Only flat DSPF files are supported; hierarchy commands,
such as .SUBCKT and .x1 are ignored.
For additional information, see “Post-Layout Back-Annotation” in the HSPICE
User Guide: RF Analysis.
Examples
In Example 1, the parasitics in the DSPF file are mapped into the hierarchical
ideal netlist.
Example 1
$ models
.MODEL p pmos
.MODEL n nmos
.INCLUDE add4.dspf
.OPTION SIM_DSPF="add4.dspf"
.VEC "dspf_adder.vec"
.TRAN 1n 5u
vdd vdd 0 3.3
.OPTION POST
.END
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
645
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF
In Example 2, the SIM_DSPF option accelerates the simulation by more than
100%. By using the SIM_LA option at the same time, you can further reduce
the total CPU time:
Example 2
$ models
.MODEL p pmos
.MODEL n nmos
.INCLUDE add4.dspf
.OPTION SIM_DSPF="add4.dspf"
.OPTION SIM_LA=PACT
.VEC "dspf_adder.vec"
.TRAN 1n 5u
vdd vdd 0 3.3
.OPTION POST
.END
Example 3, the x1.spf DSPF file is back-annotated to the x1 top-level instance.
It also back-annotates the inv.spf DSPF file to the inv subcircuit.
Example 3
.OPTION SIM_DSPF = "x1 x1.spf"
.OPTION SIM_DSPF = "inv inv.spf"
See Also
.OPTION SIM_LA
.OPTION SIM_DSPF_ACTIVE
.OPTION SIM_DSPF_SCALEC
.OPTION SIM_DSPF_SCALER
.OPTION SIM_SPEF
646
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_ACTIVE
.OPTION SIM_DSPF_ACTIVE
Runs simulation with selective DSPF expansion of active nets from one or more
DSPF files.
Syntax
.OPTION SIM_DSPF_ACTIVE=”active_node”
Description
Use this option to run simulation with selective DSPF expansion of active nets
from one or more DSPF files. HSPICE RF performs a preliminary verification
run to determine the activity of the nodes and generates two ASCII files:
active_node.rc and active_node.rcxt. These files save all active node
information in both Star-RC and Star-RCXT formats. If an active_node file is
not generated from the preliminary run, no nets are expanded. Active nets are
added to the file as they are identified in the subsequent transient simulation. A
second simulation run using the same file and option causes only the nets
listed in the active_node file to be expanded. It is possible that activity changes
are due to timing changes caused by expansion of the active nets. In this case,
additional nets are listed in the active_node file and a warning is issued.
HSPICE RF uses the active_node file and the DSPF file with the ideal netlist to
expand only the active portions of the circuit. If a net is latent, then HSPICE RF
does not expand it, which saves memory and CPU time.
For additional information, see “Selective Post-Layout Flow” in the HSPICE
User Guide: RF Analysis.
Examples
In the following example, an active net in which the tolerance of the voltage
change is greater than 0.5V is saved to both the active.rc and active.rcxt files.
Based on these files, HSPICE RF back-annotates only the active parasitics
from x1.spf and s2.spf to the x1 and x2 top-level instances.
.OPTION
.OPTION
.OPTION
.OPTION
SIM_DSPF = "x1 x1.spf"
SIM_DSPF = "x2 x2.spf"
SIM_DSPF_ACTIVE = "active"
SIM_DSPF_VTOL = 0.5V
See Also
.OPTION SIM_DSPF
.OPTION SIM_DSPF_MAX_ITER
.OPTION SIM_DSPF_VTOL
.OPTION SIM_SPEF_ACTIVE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
647
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_INSERROR
.OPTION SIM_DSPF_INSERROR
Skips unmatched instances.
Syntax
.OPTION SIM_DSPF_INSERROR=ON | OFF
Default
OFF
Description
Use this option to skip unmatched instances.
■
ON: Skips unmatched instances
■
OFF: Does not skip unmatched instances.
For additional information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
648
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_LUMPCAPS
.OPTION SIM_DSPF_LUMPCAPS
Connects a lumped capacitor with a value equal to the net capacitance for
instances missing in the hierarchical netlist.
Syntax
.OPTION SIM_DSPF_LUMPCAPS=ON | OFF
Default
ON
Description
Use this option to connect a lumped capacitor with a value equal to the net
capacitance for instances missing in the hierarchical netlist.
■
ON (default): Adds lumped capacitance while ignoring other net contents
■
OFF: Uses net contents
For additional information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
649
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_MAX_ITER
.OPTION SIM_DSPF_MAX_ITER
Specifies the maximum number of simulation runs for the second selective
DSPF expansion pass.
Syntax
.OPTION SIM_DSPF_MAX_ITER=value
Default
1
Description
Use this option to specify the maximum number of simulation runs for the
second selective DSPF expansion pass.
The value parameter specifies the number of iterations for the second
simulation run.
Some of the latent nets might turn active after the first iteration of the second
simulation run. In this case:
■
Resimulate the netlist to ensure the accuracy of the post-layout simulation.
■
Use this option to set the maximum number of iterations for the second run.
If the active_node remains the same after the second simulation run,
HSPICE RF ignores these options.
For details, see “Selective Post-Layout Flow” HSPICE User Guide: RF
Analysis.
See Also
.OPTION SIM_DSPF_ACTIVE
.OPTION SIM_DSPF_VTOL
650
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_RAIL
.OPTION SIM_DSPF_RAIL
Controls whether power-net parasitics are back-annotated
Syntax
.OPTION SIM_DSPF_RAIL=ON | OFF
Default
OFF
Description
Use this option to control whether power-net parasitics are back-annotated.
■
OFF: Do not back-annotate nets in a power rail
■
ON: Back-annotate nets in a power rail
For additional information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
651
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_SCALEC
.OPTION SIM_DSPF_SCALEC
Scales the capacitance values in a DSPF file for a standard DSPF expansion
flow.
Syntax
.OPTION SIM_DSPF_SCALEC=scaleC
Description
Use this option to scale the capacitance values in a DSPF file for a standard
DSPF expansion flow.
The scaleC parameter specifies the scale factor.
For additional information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
See Also
.OPTION SIM_LA
.OPTION SIM_DSPF_ACTIVE
652
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_SCALER
.OPTION SIM_DSPF_SCALER
Scales the resistance values in a DSPF file for a standard DSPF expansion
flow.
Syntax
.OPTION SIM_DSPF_SCALER=scaleR
Description
Use this option to scale the resistance values in a DSPF file for a standard
DSPF expansion flow.
The scaleR specifies the scale factor.
For additional information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
See Also
.OPTION SIM_LA
.OPTION SIM_DSPF_ACTIVE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
653
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_VTOL
.OPTION SIM_DSPF_VTOL
Specifies multiple DSPF active thresholds.
Syntax
.OPTION SIM_DSPF_VTOL=“value | scope1 scope2 ...
+ scopen”
Default 0.1V
Description
Use this option to specify multiple DSPF active thresholds.
■
The value parameter specifies the tolerance of voltage change. This value
should be relatively small compared to the operating range of the circuit or
smaller than the supply voltage.
■
scopen can be a subcircuit definition that uses a prefix of “@” or a subcircuit
instance.
HSPICE RF performs a second simulation run by using the active_node file,
the DSPF, and the hierarchical LVS ideal netlist to back-annotate only active
portions of the circuit. If a net is latent, HSPICE RF does not expand the net.
This saves simulation runtime and memory.
By default, HSPICE RF performs only one iteration of the second simulation
run. Use the SIM_DSPF_MAX_ITER option to change this setting.
For additional information, see “Selective Post-Layout Flow” in the HSPICE
User Guide: RF Analysis.
Examples
In Example 1, the first line sets the sensitivity voltage to 0.01V. Subcircuit
definition snsamp and the subcircuit instance xvco have full parasitics if their
nodes move more than 0.01V during active nodes generation. In the second
line, xand and xff are less sensitive than the default, indicating that they are not
sensitive to parasitics.
Example 1
.OPTION SIM_DSPF_VTOL=“0.01 | @snsamp xvco”
.OPTION SIM_DSPF_VTOL=“0.25 | xand xff”
654
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_DSPF_VTOL
In this example, the sense amp circuit uses full parasitics if their nodes move
more than 0.01V during active-node generation. The inv subcircuit definition is
less sensitive than the default so the nodes are less sensitive to the parasitics.
Example 2
.OPTION SIM_DSPF = "inv inv.spf"
.OPTION SIM_DSPF = "senseamp senseamp.spf"
.OPTION SIM_DSPF_ACTIVE = "activenet"
.OPTION SIM_DSPF_VTOL = "0.15 | @inv"
.OPTION SIM_DSPF_VTOL = "0.01 | @senseamp"
See Also
.OPTION SIM_DSPF_ACTIVE
.OPTION SIM_DSPF_MAX_ITER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
655
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_LA
.OPTION SIM_LA
Activates linear matrix (RC) reduction for HSPICE/HSPICE RF.
Syntax
.OPTION SIM_LA=[PACT | PI | 0 | 1 | 2 ]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to activate linear matrix reduction. SIM_LA does not reduce a
node used by any analysis command, such as .PROBE, .MEASURE, and so on
This option accelerates the simulation of circuits that include large linear RC
networks by reducing all matrixes that represent RC networks.
■
0 turns off SIM_LA
■
1 is the equivalent of PACT, which selects the Pole Analysis via Congruence
Transforms (PACT) algorithm to reduce RC networks in a well-conditioned
manner, while preserving network stability.
■
2 invokes the PI algorithm to create PI models of the RC networks.
■
If SIM_LA is not specified in the input file, the lis file returns SIM_LA=0.
■
If SIM_LA is specified with no value or SIM_LA=PACT, the lis file returns
SIM_LA=1.
■
If SIM_LA=PI, the lis file returns SIM_LA=2.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: Simulation and Analysis or “Linear Acceleration” in the HSPICE User
Guide: RF Analysis.
See Also
.OPTION SIM_DSPF
.OPTION LA_FREQ
.OPTION LA_MAXR
.OPTION LA_MINC
.OPTION LA_TIME
.OPTION LA_TOL
656
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_LA_FREQ
.OPTION SIM_LA_FREQ
Specifies the upper frequency for which accuracy must be preserved.
Syntax
.OPTION SIM_LA_FREQ=value
Default
1GHz
Description
Use this option to specify the upper frequency for which accuracy must be
preserved. The value parameter specifies the upper frequency for which the
PACT algorithm must preserve accuracy. If value is 0, the algorithm drops all
capacitors because only DC is of interest.
The maximum frequency required for accurate reduction depends on both the
technology of the circuit and the time scale of interest. In general, the faster the
circuit, the higher the maximum frequency. For additional information, see
“Linear Acceleration” in the HSPICE User Guide: RF Analysis.
See Also
.OPTION SIM_LA
.OPTION SIM_LA_TIME
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
657
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_LA_MAXR
.OPTION SIM_LA_MAXR
Specifies the maximum resistance for linear matrix reduction.
Syntax
.OPTION SIM_LA_MAXR=value
Default
1e15 ohms
Description
Use this option to specify the maximum resistance for linear matrix reduction.
The value parameter specifies the maximum resistance preserved in the
reduction. The linear matrix reduction process assumes that any resistor
greater than value has an infinite resistance and drops the resistor after
reduction completes. For additional information, see “Linear Acceleration” in
the HSPICE User Guide: RF Analysis.
See Also
.OPTION SIM_LA
658
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_LA_MINC
.OPTION SIM_LA_MINC
Specifies the minimum capacitance for linear matrix reduction.
Syntax
.OPTION SIM_LA_MINC=value
Default
1e-16 farads
Description
Use this option to specify the minimum capacitance for linear matrix reduction.
The value parameter specifies the minimum capacitance preserved in the
reduction.
The linear matrix reduction process lumps any capacitor smaller than value to
ground after the reduction completes.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: RF Analysis.
See Also
.OPTION SIM_LA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
659
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_LA_TIME
.OPTION SIM_LA_TIME
Specifies the minimum time for which accuracy must be preserved.
Syntax
.OPTION SIM_LA_TIME=value
Default
1 ns.
Description
Use this option to specify the minimum time for which accuracy must be
preserved.
The value parameter specifies the minimum switching time for which the PACT
algorithm preserves accuracy.
Waveforms that occur more rapidly than the minimum switching time are not
accurately represented.
This option is simply an alternative to .OPTION SIM_LA_FREQ. The default is
equivalent to setting SIM_LA_FREQ=1GHz.
Note:
Higher frequencies (smaller times) increase accuracy, but only
up to the minimum time step used in HSPICE RF.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: RF Analysis.
Examples
For a circuit having a typical rise time of 1ns, either set the maximum frequency
to 1 GHz, or set the minimum switching time to 1ns:
.OPTION SIM_LA_FREQ=1GHz
-or.OPTION SIM_LA_TIME=1ns
However, if spikes occur in 0.1ns, HSPICE RF does not accurately simulate
them. To capture the behavior of the spikes, use:
.OPTION SIM_LA_FREQ=10GHz
-or.OPTION SIM_LA_TIME=0.1ns
See Also
.OPTION SIM_LA
.OPTION SIM_LA_FREQ
660
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_LA_TOL
.OPTION SIM_LA_TOL
Specifies the error tolerance for the PACT algorithm.
Syntax
.OPTION SIM_LA_TOL=value
Default 0.05ns.
Description
Use this option to specify the error tolerance for the PACT algorithm.
The value parameter must specify a real number between 0.0 and 1.0.
For additional information, see “Linear Acceleration” in the HSPICE User
Guide: RF Analysis.
See Also
.OPTION SIM_LA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
661
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_ORDER
.OPTION SIM_ORDER
Controls the amount of Backward-Euler (BE) method to mix with the
Trapezoidal (TRAP) method for hybrid integration.
Syntax
.OPTION SIM_ORDER=x
Default 1.9
Description
Use this option to control the amount of Backward-Euler (BE) method to mix
with the Trapezoidal (TRAP) method for hybrid integration.
The x parameter must specify a real number between 1.0 and 2.0.
■
SIM_ORDER=1.0 selects BE
■
SIM_ORDER=2.0 selects TRAP.
Note: .OPTION SIM_ORDER has precedence over .OPTION
SIM_TRAP.
A higher order is more accurate, especially with inductors (such as crystal
oscillators), which need SIM_ORDER=2.0. A lower order has more damping.
This option affects time stepping when you set .OPTION METHOD to TRAP or
TRAPGEAR.
Examples
This example causes a mixture of 10% Gear-2 and 90% BE-trapezoidal hybrid
integration. The BE-trapezoidal part is 10% BE.
.option sim_order=1.9
See Also
.OPTION METHOD
.OPTION SIM_TRAP
662
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_OSC_DETECT_TOL
.OPTION SIM_OSC_DETECT_TOL
Specifies the tolerance for detecting numerical oscillations.
Syntax
.OPTION SIM_OSC_DETECT_TOL=value
Default 10^8
Description
Use this option to specify the tolerance for detecting numerical oscillations. If
HSPICE RF detects numerical oscillations, it inserts Backward-Euler (BE)
steps. Smaller values of this tolerance result in fewer BE steps.
See Also
.OPTION METHOD
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
663
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POSTAT
.OPTION SIM_POSTAT
Limits waveform output to nodes in the specified subcircuit instance.
Syntax
.OPTION SIM_POSTAT=instance
Description
Use this option to limit waveform output to nodes in the specified subcircuit
instance only. SIM_POSTAT is available for both HSPICE and HSPICE RF.
Wildcards are supported.
Examples
The following example outputs X1.X4; see Figure 15.
.OPTION SIM_POSTAT=X1.X4
top
X1(ADD)
Figure 15
X5
X4
X3
X1
X2(SUB)
X2
X1
X6
X2
Node Hierarchy
See Also
.OPTION SIM_POSTSKIP
.OPTION SIM_POSTTOP
664
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POSTDOWN
.OPTION SIM_POSTDOWN
Limits waveform output to nodes in the specified subcircuit instance and their
children.
Syntax
.OPTION SIM_POSTDOWN=instance
Description
Use this option with .OPTION SIM_POSTTOP and it takes precedence over
.OPTION SIM_POSTSKIP.
Wildcards are supported.
Examples
The following example outputs top, X1, X1.X4, X1.X4.X1, X1.X4.X2, and X2.
(See Figure 15 on page 664.)
.OPTION SIM_POSTTOP=2
.OPTION SIM_POSTDOWN=X1.X4
See Also
.OPTION SIM_POSTAT
.OPTION SIM_POSTSKIP
.OPTION SIM_POSTTOP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
665
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POSTSCOPE
.OPTION SIM_POSTSCOPE
Specifies the signal types to probe from within a scope.
Syntax
.OPTION SIM_POSTSCOPE= net | port | all
Description
Use this option to specify the signal types to probe from within a scope.
■
net: Outputs only nets in the scope
■
port: Outputs both nets and ports
■
all: Outputs nets, ports, and global variables.
See Also
.OPTION POST
.OPTION SIM_POSTSKIP
.OPTION SIM_POSTTOP
666
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POSTSKIP
.OPTION SIM_POSTSKIP
Causes the SIM_POSTTOP option to skip subckt_definition instances.
Syntax
.OPTION SIM_POSTSKIP=subckt_definition
Description
Use this option to cause the SIM_POSTTOP option to skip any instances and
their children that are defined by the subckt_definition parameter. To specify
more than one subcircuit definition, issue this option once for each definition
you want to skip. SIM_POSTSKIP is available for both HSPICE and HSPICE
RF. Wildcards are supported.
Examples
The following example outputs top, and skips X2. X1 because they are
instances of the ADD subcircuit. (See Figure 15 on page 664.)
.OPTION SIM_POSTTOP=2
.OPTION SIM_POSTSKIP=ADD
See Also
.OPTION SIM_POSTTOP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
667
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POSTTOP
.OPTION SIM_POSTTOP
Limits data written to your waveform file to data from only the top n level nodes.
Syntax
.OPTION SIM_POSTTOP=n
Description
Limits the data written to your waveform file to data from only the top n level
nodes. SIM_POSTAT is available for both HSPICE and HSPICE RF.
This option outputs instances from up to n levels deep.
■
SIM_POSTTOP=3: Outputs instances from 3 levels deep
■
SIM_POSTTOP=1: Outputs instances from only the top-level signals.
If you specify the PROBE option without specifying a SIM_POSTTOP option
HSPICE RF sets the SIM_POSTTOP=0. HSPICE RF outputs all levels if you do
not specify either the PROBE option or a SIM_POSTTOP option.
Wildcards are not currently supported.
Note:
You must specify the POST option to enable the waveform display
interface.
SIM_POSTTOP is equivalent POSTTOP used in HSPICE.
Examples
Example 1 outputs top, X1, and X2. (See Figure 15 on page 664.)
Example 1
.OPTION SIM_POSTTOP=2
The following example outputs top, X1, X2,and X4, X1and X2. (See Figure 15
on page 664.)
Example 2
.OPTION SIM_POSTTOP=2
.OPTION SIM_POSTDOWN=X1.X4
See Also
.OPTION POST
.OPTION PROBE
.OPTION SIM_POSTSKIP
668
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWER_ANALYSIS
.OPTION SIM_POWER_ANALYSIS
Prints a list of signals matching the tolerance setting at a specified point in time.
Syntax
.OPTION SIM_POWER_ANALYSIS=“time_pointtol”
.OPTION SIM_POWER_ANALYSIS=“bottom time_pointtol”
Argument
Description
time_point
Time when HSPICE RF detects signals where the port current is
larger than the tolerance value.
tol
Tolerance value for the signal defined in the .POWER command.
bottom
Signal at the lowest hierarchy level, also called a leaf subcircuit.
Description
Use this option to print a list of signals matching the tolerance (tol) setting at
a specified point in time.
The first syntax produces a list of signals that consume more current than tol
at time point, in this format:
The second syntax produces the list of lowest-level signals, known as leaf
subcircuits that consume more than tol at time point. The output is similar
to this:
For additional information, see “Power Analysis Output Format” in the HSPICE
User Guide: RF Analysis.
Examples
In this example, print the names of leaf subcircuits that use more than 100uA at
100ns into the simulation are printed.
.OPTION SIM_POWER_ANALYSIS=“bottom 100ns 100ua”
.POWER VDD
See Also
.POWER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
669
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWER_TOP
.OPTION SIM_POWER_TOP
Controls the number of hierarchy levels on which power analysis is performed.
Syntax
.OPTION SIM_POWER_TOP=value
Description
Use this option to control the number of hierarchy levels on which power
analysis is performed.
By default, power analysis is performed on the top levels of hierarchy.
Examples
In the following example, HSPICE RF produces .POWER command results for
top-level and first-level subcircuits (the subcircuit children of the top-level
subcircuits).
.OPTION SIM_POWER_TOP=2
See Also
.POWER
670
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWERDC_ACCURACY
.OPTION SIM_POWERDC_ACCURACY
Increases the accuracy of operating point calculations for POWERDC analysis.
Syntax
.OPTION SIM_POWERDC_ACCURACY=value
Description
Use this option to increase the accuracy of operating point calculations for
POWERDC analysis.
A higher value results in greater accuracy, but more time to complete the
calculation.
See Also
.POWERDC
.OPTION SIM_POWERDC_HSPICE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
671
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWERDC_HSPICE
.OPTION SIM_POWERDC_HSPICE
Increases the accuracy of operating point calculations for POWERDC analysis.
Syntax
.OPTION SIM_POWERDC_HSPICE
Description
Use this option to increase the accuracy of operating point calculations for
POWERDC analysis.
See Also
.POWERDC
.OPTION SIM_POWERDC_ACCURACY
672
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWERPOST
.OPTION SIM_POWERPOST
Controls power analysis waveform dumping.
Syntax
.OPTION SIM_POWERPOST=ON|OFF
Description
Use this option to enable or disable power analysis waveform dumping.
See Also
.POWER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
673
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWERSTART
.OPTION SIM_POWERSTART
Specifies a default start time for measuring signals during simulation.
Syntax
.OPTION SIM_POWERSTART=time
Description
Use this option with a .POWER command to specify a default start time for
measuring signals during simulation. This default time applies to all signals that
do not have their own FROM measurement time. This option together with the
.OPTION SIM_POWERSTOP control the power measurement scope for an
entire simulation.
Examples
In this example, the scope for simulating the x1.in signal is from 10 ps to 90 ps.
.OPTION SIM_POWERSTART=10ps
.OPTION SIM_POWERSTOP=90ps
.power x1.in
See Also
.OPTION SIM_POWERSTOP
.OPTION SIM_POWERSTART
674
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_POWERSTOP
.OPTION SIM_POWERSTOP
Specifies a default stop time for measuring signals during simulation.
Syntax
.OPTION SIM_POWERSTOP=time
Description
Use this option with a .POWER command to specify a default stop time for
measuring signals during simulation. This default time applies to all signals that
do not have their own TO measurement time. This option together with the
.OPTION SIM_POWERSTART control the power measurement scope for an
entire simulation.
See Also
.OPTION SIM_POWERSTART
.POWER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
675
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF
.OPTION SIM_SPEF
Runs simulation with SPEF expansion of all nets from one or more SPEF files.
Syntax
.OPTION SIM_SPEF=“spec_filename”
Description
Use this option to run simulation with SPEF expansion of all nets from one or
more SPEF files.
You can repeat this option to include more SPEF files.
For additional information, see “Post-Layout Back-Annotation” in the HSPICE
User Guide: RF Analysis.
Examples
In this example, the senseamp.spf SPEF file is back-annotated to the sense
amp circuit.
.OPTION SIM_SPEF = "senseamp.spf"
See Also
.OPTION SIM_SPEF_ACTIVE
.OPTION SIM_SPEF_SCALEC
.OPTION SIM_SPEF_SCALER
676
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_ACTIVE
.OPTION SIM_SPEF_ACTIVE
Runs simulation with selective SPEF expansion of active nets from one or more
DSPF files.
Syntax
.OPTION SIM_SPEF_ACTIVE=”active_node”
Description
Use this option to run simulation with selective SPEF expansion of active nets
from one or more DSPF files.
HSPICE RF performs a preliminary verification run to determine the activity of
the nodes and generates two ASCII files: active_node.rc and active_node.rcxt.
These files save all active node information in both Star-RC and Star-RCXT
formats.
If an active_node file is not generated from the preliminary run, no nets are
expanded. Active nets are added to the file as they are identified in the
subsequent transient simulation. A second simulation run using the same file
and option causes only the nets listed in the active_node file to be expanded. It
is possible that activity changes are due to timing changes caused by
expansion of the active nets. In this case, additional nets are listed in the
active_node file and a warning is issued.
By default, a node is considered active if the voltage varies by more than 0.1 V.
You can use the SIM_SPEF_VTOL option to change this value.
HSPICE RF uses the active_node file and the DSPF file with the ideal netlist to
expand only the active portions of the circuit. If a net is latent, then HSPICE RF
does not expand it, which saves memory and CPU time.
For additional information, see “Selective Post-Layout Flow” in the HSPICE
User Guide: RF Analysis.
See Also
.OPTION SIM_SPEF_VTOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
677
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_INSERROR
.OPTION SIM_SPEF_INSERROR
Skips unmatched instances.
Syntax
.OPTION SIM_SPEF_INSERROR=ON | OFF
Description
Use this option to skip unmatched instances.
■
ON: Skips unmatched instances.
■
OFF: Does not skip unmatched instances.
For more information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
678
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_LUMPCAPS
.OPTION SIM_SPEF_LUMPCAPS
Connects a lumped capacitor with a value equal to the net capacitance for
instances missing in the hierarchical netlist.
Syntax
.OPTION SIM_SPEF_LUMPCAPS=ON | OFF
Description
Use this option to connect a lumped capacitor with a value equal to the net
capacitance for instances missing in the hierarchical netlist.
■
ON: Adds lumped capacitance while ignoring other net contents.
■
OFF: Uses net contents.
For additional information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
679
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_MAX_ITER
.OPTION SIM_SPEF_MAX_ITER
Specifies the maximum number of simulation runs for the second selective
SPEF expansion pass.
Syntax
.OPTION SIM_SPEF_MAX_ITER=value
Description
Use this option to specify the maximum number of simulation runs for the
second selective SPEF expansion pass.
The value parameter specifies the number of iterations for the second
simulation run.
Some of the latent nets might turn active after the first iteration of the second
simulation run. In this case:
■
Re simulate the netlist to ensure the accuracy of the post-layout simulation.
■
Use this option to set the maximum number of iterations for the second run.
If the active_node remains the same after the second simulation run,
HSPICE RF ignores these options.
For additional information, see “Selective Post-Layout Flow” in the HSPICE
User Guide: RF Analysis.
See Also
.OPTION SIM_SPEF_ACTIVE
.OPTION SIM_SPEF_VTOL
680
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_PARVALUE
.OPTION SIM_SPEF_PARVALUE
Interprets triplet format float:float:float values in SPEF files as
best:average:worst.
Syntax
.OPTION SIM_SPEF_PARVALUE=1|2|3
Description
Use this option to interpret triplet format float:float:float values in SPEF files as
best:average:worst.
■
SIM_SPEF_PARVALUE = 1: Use best.
■
SIM_SPEF_PARVALUE = 2: Use average.
■
SIM_SPEF_PARVALUE = 3: Use worst.
For further information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
681
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_RAIL
.OPTION SIM_SPEF_RAIL
Controls whether power-net parasitics are back-annotated.
Syntax
.OPTION SIM_SPEF_RAIL=ON | OFF
Description
Use this option to control whether power-net parasitics are back-annotated.
■
OFF: Do not back-annotate nets in a power rail.
■
ON: Back-annotate nets in a power rail.
For further information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
682
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_SCALEC
.OPTION SIM_SPEF_SCALEC
Scales the capacitance values in a SPEF file for a standard SPEF expansion
flow.
Syntax
.OPTION SIM_SPEF_SCALEC=scaleC
Description
Use this option to scale the capacitance values in a SPEF file for a standard
SPEF expansion flow.
The scaleC parameter specifies the scale factor.
See “Additional Post-Layout Options” in the HSPICE User Guide: RF Analysis.
See Also
.OPTION SIM_SPEF_ACTIVE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
683
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_SCALER
.OPTION SIM_SPEF_SCALER
Scales the resistance values in a SPEF file for a standard SPEF expansion
flow.
Syntax
.OPTION SIM_SPEF_SCALER=scaleR
Description
Use this option to scale the resistance values in a SPEF file for a standard
SPEF expansion flow.
The scaleR parameter specifies the scale factor.
For more information, see “Additional Post-Layout Options” in the HSPICE
User Guide: RF Analysis.
See Also
.OPTION SIM_SPEF_ACTIVE
684
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_SPEF_VTOL
.OPTION SIM_SPEF_VTOL
Specifies multiple SPEF active thresholds.
Syntax
.OPTION SIM_SPEF_VTOL=“value | scope1 scope2...
+ scopen”
Description
Use this option to specify multiple SPEF active thresholds.
■
The value parameter specifies the tolerance of voltage change. This value
should be relatively small compared to the operating range of the circuit, or
smaller than the supply voltage.
■
The scopen parameter can be a subcircuit definition that uses a prefix of “@”
or a subcircuit instance.
HSPICE RF performs a second simulation run by using the active_node file,
the SPEF, and the hierarchical LVS ideal netlist to back-annotate only active
portions of the circuit. If a net is latent, then HSPICE RF does not expand the
net. This saves simulation runtime and memory.
By default, HSPICE RF performs only one iteration of the second simulation
run. Use the SIM_SPEF_MAX_ITER option to change it.
For additional information, see “Selective Post-Layout Flow” in the HSPICE
User Guide: RF Analysis.
See Also
.OPTION SIM_SPEF_ACTIVE
.OPTION SIM_SPEF_MAX_ITER
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
685
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_TG_THETA
.OPTION SIM_TG_THETA
Controls the amount of second-order Gear method to mix with Trapezoidal
integration for the hybrid TRAPGEAR method.
Syntax
.OPTION SIM_TG_THETA=[0|1]
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to control the amount of second-order Gear (Gear-2) method to
mix with Trapezoidal (TRAP) integration for the hybrid TRAPGEAR method.
The value parameter must specify a value between 0.0 and 1.0. The default
is 0.1.
■
SIM_TG_THETA=0 selects TRAP without Gear-2.
■
SIM_TG_THETA=1 selects pure Gear-2.
See Also
.OPTION METHOD
686
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SIM_TRAP
.OPTION SIM_TRAP
Changes the default SIM_TG_THETA=0 so that METHOD=TRAPGEAR acts like
METHOD=TRAP.
Syntax
.OPTION SIM_TRAP=x
Description
Use this option to change the default SIM_TG_THETA=0 so that
METHOD=TRAPGEAR acts like METHOD=TRAP.
The x parameter must specify a value between 0.0 and 1.0.
See Also
.OPTION METHOD
.OPTION SIM_TG_THETA
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
687
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SI_SCALE_SYMBOLS
.OPTION SI_SCALE_SYMBOLS
Controls whether the scale factors are HSPICE attributes or International
System of Units (SI) when case sensitivity is invoked.
Syntax
SI_SCALE_SYMBOLS=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
SI_SCALE_SYMBOLS=1 changes the scaling factors from the HSPICE
standard (default) to the International System of Units (SI) to enable you to use
case sensitive scaling symbols. (Using the (=1) setting assures consistency
with spice scale factors for downstream tools.)
Note:
Multiplying
Factors
This option is enabled when case-sensitivity is on (-case 1).
Description
.OPTION_SCALE_SYMBOLS=S
%> hspice -case C
S=0, C=0 (default)
S=0, C=1
(Same as
S=0, C=0)
S=1, C=1
1e12
Tera
T, t
T, t
1e9
Giga
G, g
G, g
1e6
Mega
MEG, meg, X, x
M, MEG, meg, X, X
1e3
Kilo
K, k
K, k
1e-3
Milli
M or m
m
25.4e-6
1,000(s) of
an inch
MIL, mil
MIL, mil
1e-6
Mico
U, u
U, u
1e-9
Nano
N, n
N, n
1e-12
Pico
P, p
P, p
1e-15
Femto
F, f
F, f
1e-18
Atto
A, a
A, a
S=1, C=0
Same as
S=0,C=0
See Also
.OPTION PCB_SCALE_FORMAT
688
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SLOPETOL
.OPTION SLOPETOL
Specifies the minimum value for breakpoint table entries in a piecewise linear
(PWL) analysis.
Syntax
.OPTION SLOPETOL=x
Description
Use this option to specify the minimum value for breakpoint table entries in a
piecewise linear (PWL) analysis. If the difference in the slopes of two
consecutive PWL segments is less than the SLOPETOL value, HSPICE RF
ignores the breakpoint for the point between the segments. Min value: 0; Max
value: 2.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
689
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SNACCURACY
.OPTION SNACCURACY
Sets and modifies the size of timesteps.
Syntax
.OPTION SNACCURACY=integer
Default
10
Description
Use this option to set and modify the size of timesteps. Larger values of
snaccuracy result in a more accurate solution but might require more time
points. Because Shooting-Newton must store derivative information at every
time point, the memory requirements might be significant if the number of time
points is very large. The maximum integer value is 50.
For additional information, see SN Steady-State Time Domain Analysis in the
HSPICE User Guide: RF Analysis.
See Also
.OPTION SIM_ACCURACY
.OPTION SNMAXITER (or) SN_MAXITER
690
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SNCONTINUE
.OPTION SNCONTINUE
Specifies whether to use the sweep solution from the previous simulation as
the initial guess for the present simulation.
Syntax
.OPTION SNCONTINUE= 0|1
Default
1
Description
Use this option to specify whether to use the sweep solution from the previous
simulation as the initial guess for the present simulation.
■
SNCONTINUE=1: Use solution from previous simulation as the initial guess.
■
SNCONTINUE=0: Start each simulation in a sweep from the DC solution.
See Also
.SN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
691
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SNMAXITER (or) SN_MAXITER
.OPTION SNMAXITER (or) SN_MAXITER
Sets the maximum number of iterations for a Shooting Newton analysis.
Syntax
.OPTION SNMAXITER | SN_MAXITER=integer
Description
Use this option to limit the number of SN iterations. For more information, see
Steady-State Shooting Newton Analysis in the HSPICE User Guide: RF
Analysis.
See Also
.SN
692
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SOIQ0
.OPTION SOIQ0
Invokes the body charge initialization (BQI) algorithm.
Syntax
.OPTION SOIQ0=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to invoke the BQI algorithm for floating body SOI transistors.
This option is to be used in conjunction with instance parameter soiq0.
The BQI algorithm allows users to specify a SOI device initial state for
simulation to start with the initial state. The initial body charge can be provided
by CFL function calls.
The BQI algorithm is applied to SOI models (Levels: 57, 60, and 70). For
additional information, see MOSFET Models (BSIM): Levels 47 through 72 in
the HSPICE Reference Manual: MOSFET Models.
See Also
.DC
.OP
.TRAN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
693
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SPLIT_DP
.OPTION SPLIT_DP
Enables the writing of multiple operating points in separate files.
Syntax
.OPTION SPLIT_DP=0|1|2
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option in conjunction with .OPTION OPFILE when back annotating
the operating point information for the Synopsys Custom Designer product.
■
If .OPTION SPLIT_DP=0, HSPICE ignores the SPLIT_DP option.
■
If OPFILE=1 and SPLIT_DP=0, HSPICE writes operating point information
for all time points specified in the .OP statement in a single .dp0 file. If
OPFILE=1 and SPLIT_DP=1, HSPICE writes operating point information in
a separate file for each time point specified in .OP statement.
■
If OPFILE=2.op0 and .dp0 files are created together except that with sweep
variables, split_dp=2 permits you to create *.op0 files corresponding to
*.dp0 files with sweep.
Note: Because the split_dp=2 option was developed for the
Custom Designer Environment, HSPICE users should avoid
its use lest you create more *.dp0 and *.op0 files than you
desire.
Examples
The following command, these files below are returned:
.option opfile=1 split_dp=2
*.op0
*.dp0
*[email protected]@sweep_index
*[email protected]@sweep_index
With .op timepoint1 timepoint2... in the netlist,
.tran '1n' '2n' start='0' sweep monte=10 firstrun=1
.option opfile=1 split_dp=1
The resulting files are generated:
694
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SPLIT_DP
*.op0
*.dp0
*[email protected]@sweep_index
See Also
.OPTION OPFILE
.OPTION WDF
.OP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
695
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SPMODEL
.OPTION SPMODEL
Disables the previous .OPTION VAMODEL.
Syntax
.OPTION SPMODEL [= name]
Description
Use this option to disable a previously issued VAMODEL option. In this option,
the name is the cell name that uses a SPICE definition. Each SPMODEL option
can take no more than one name. Multiple names need multiple SPMODEL
options.
Examples
Example 1 disables the previous .OPTIONVAMODEL but has no effect on the
other VAMODEL options if they are specified for the individual cells. For
example, if .OPTIONVAMODEL=vco has been set, the vco cell uses the
Verilog-A definition whenever it is available until .OPTIONSPMODEL=vco
disables it.
.OPTION SPMODEL
This example disables the previous .OPTIONVAMODEL=chargepump, which
causes all instantiations of chargepump to now use the subcircuit definition
again.
.option spmodel=chargepump
See Also
.OPTION VAMODEL
696
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION STATFL
.OPTION STATFL
Controls whether HSPICE creates a .st0 file.
Syntax
.OPTION STATFL=0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
Use this option to control whether HSPICE creates a .st0 file.
■
STATFL=0 Outputs a .st0 file.
■
STATFL=1 Suppresses the .st0 file.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
697
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION STRICT_CHECK
.OPTION STRICT_CHECK
Turns a subset of HSPICE netlist syntax warnings into terminal (abortive)
syntax errors.
Syntax
.OPTION STRICT_CHECK 0|1
Default Value if option is not specified in the netlist: 0
Value if option name is specified without a corresponding value: 1
Description
When enabled (set to 1), netlist conditions listed below will abort HSPICE with
an error message. When disabled (set to 0), HSPICE will make assumptions
and continue to run with only a warning message.
The following is a list of the messages controlled by STRICT_CHECK:
10001, 10002, 10003,10004, 10008, 10011, 10012, 10013, 10018, 10019,
10020, 10021, 10047, 10048. For more information refer to Warning Message
Index [10001-10076] located in the HSPICE User Guide: Simulation and
Analysis, Chapter 34, Warning/Error Messages.
See Also
.OPTION MESSAGE_LIMIT
698
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SX_FACTOR
.OPTION SX_FACTOR
External shrink factor, only used for Ivthx calculation with the .IVTH command.
Syntax
.IVTH model_name Ivth0=x DW=x DL=x
.OPTION SX_factor=x
Description
This option is only used with the IVTH command as shown in the Syntax
section. It is restricted to use for ivthx calculation only.
See Also
.IVTH
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
699
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION SYMB
.OPTION SYMB
Uses a symbolic operating point algorithm to get initial guesses before
calculating operating points.
Syntax
.OPTION SYMB=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to calculate the operating point. When SYMB is set to 1,
HSPICE operates with a symbolic operating point algorithm to get initial
guesses before calculating operating points. SYMB assumes the circuit is digital
and assigns a low/high state to all nodes that set a reasonable initial voltage
guess. This option improves DC convergence for oscillators, logic, and mixedsignal circuits.
.OPTION SYMB does not have any effect on the transient analysis if you set
UIC in the .TRAN command.
700
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TIMERES
.OPTION TIMERES
Sets the minimum separation between breakpoint values for the breakpoint
table.
Syntax
.OPTION TIMERES=x
Description
Use this option to set the minimum separation between breakpoint values for
the breakpoint table. If two breakpoints are closer together in time than the
TIMERES value, HSPICE enters only one of them in the breakpoint table.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
701
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TMIFLAG
.OPTION TMIFLAG
Invokes the TSMC Model Interface (TMI) flow.
Syntax
.OPTION TMIFLAG=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to invoke the TMI flow using proprietary TSMC model files and
compiled libraries. The TMIFLAG option must equal 1 to enable a TMI flow.
Both the technology and API are jointly developed by Synopsys and TSMC.
The TMI is a compact model with additional instance parameters and equations
to support TSMC’s extension of the standard BSIM4 model. Modeling API code
is written in C and available in a compiled format for HSPICE and HSIM to link
to during the simulation. TMI-required settings to invoke the flow and the
location of a .so file are set by TSMC using their TMIMODEL parameter with the
HSPICE TMI. The API also performs automatic platform selection on the .so
file. Both HSPICE and HSIM provide the tool binaries and support the same .so
file. To point to a TMI .so file location use the .OPTION TMIPATH command.
If .OPTION TMIFLAG=1, .OPTION MACMOD automatically equals 3 to enable
the mapping of an instance name starting with “x” to “m” thus allowing TMI
libraries to be shared for all vendor's simulator(s).
Use the existing HSPICE and HSIM commands to run the simulation. (Contact
Synopsys Technical Support for further information.)
See Also
.OPTION TMIPATH
.OPTION MACMOD
702
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TMIPATH
.OPTION TMIPATH
Points to a TMI *.so (compiled library) file location.
Syntax
.OPTION TMIPATH=‘tmifilename_dir’
Description
Use this option to point to a TSMC Model Interface (TMI) *.so file location. The
path must be enclosed in single quotation marks. This option supports both
relative and absolute paths.
Examples
.option tmipath=‘tmi_v0d03_dir’
See Also
.OPTION TMIFLAG
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
703
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TMIVERSION
.OPTION TMIVERSION
Specifies TMI version.
Syntax
.OPTION TMIVERSION=1.0|2.0
Default 1.0
Description
Use this option to select the TMI version:
704
■
1.0: Compatible with version TMI 1. HSPICE passes the model level and
model type id (e.g., TMI_MOS_MODEL in tmiDef.h) to TMI for TMI model
selection
■
2.0: Compatible with TMI 2 and CMC TMI. HSPICE passes model name id
(e.g,. TMI_MOS_BSIM4, TMI_MOS_PSP... defined in tmiDef.h) to TMI
for TMI model selection.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TNOM
.OPTION TNOM
Sets the reference temperature for the simulation.
Syntax
.OPTION TNOM=x
Default
25°C
Description
Use this option to set the reference temperature for the HSPICE RF simulation.
At this temperature, component derating is zero.
Note:
The reference temperature defaults to the analysis temperature
if you do not explicitly specify a reference temperature.
See Also
.TEMP (or) .TEMPERATURE
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
705
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TRANFORHB
.OPTION TRANFORHB
Forces HB analysis to recognize or ignore specific V/I sources.
Syntax
.OPTION TRANFORHB=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
This option forces HB analysis to recognize or ignore specific V/I sources.
■
TRANFORHB=1: Forces HB analysis to recognize V/I sources that include
SIN, PULSE, VMRF, and PWL transient descriptions, and to use them in
analysis. However, if the source also has an HB description, analysis uses
the HB description instead.
■
TRANFORHB=0: Forces HB to ignore transient descriptions of V/I sources
and to use only HB descriptions.
To override this option, specify TRANFORHB in the source description.
See Also
.HB
706
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TRCON
.OPTION TRCON
Controls the automatic convergence process of transient simulation.
Syntax
.OPTION TRCON=[0|1|2]
Default
1
Description
Use this option to control autoconvergence of transient simulation. If the circuit
fails to converge using the default trapezoidal (TRAP) numerical integration
method (for example because of trapezoidal oscillation), HSPICE sets the
GEAR method to run the transient simulation again from time=0. This process
is autoconvergence. If HSPICE fails to converge, an “internal timestep too
small” error is issued.
■
TRCON=0: Disables autoconvergence.
■
TRCON=1: Enables autoconvergence for transient simulation only when the
accumulated CPU time of the current simulation is less than 1 hour.
■
TRCON=2: Enables autoconvergence with no restriction; in addition, a
simulation enters into transient analysis without a converged operating
point.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
707
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION TRTOL
.OPTION TRTOL
Estimates the amount of error introduced when the timestep algorithm
truncates the Taylor series expansion.
Syntax
.OPTION TRTOL=x
Description
Use this option timestep algorithm for local truncation error
(LVLTIM=2).HSPICE multiplies TRTOL by the internal timestep, which is
generated by the timestep algorithm for the local truncation error. TRTOL
reduces simulation time and maintains accuracy. It estimates the amount of
error introduced when the algorithm truncates the Taylor series expansion. This
error reflects the minimum timestep to reduce simulation time and maintain
accuracy.
The range of TRTOL is 0.01 to 100; typical values are 1 to 10. If you set TRTOL
to 1 (the minimum value), HSPICE uses a very small timestep. As you increase
the TRTOL setting, the timestep size increases.
See Also
.OPTION LVLTIM
708
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION UNWRAP
.OPTION UNWRAP
Displays phase results for AC analysis in unwrapped form.
Syntax
.OPTION UNWRAP=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to display phase results for AC analysis in unwrapped form
(with a continuous phase plot).HSPICE uses these results to accurately
calculate group delay. HSPICE also uses unwrapped phase results to compute
group delay, even if you do not set UNWRAP. By default, HSPICE calculates the
unwrapped phase first and then converts it to wrapped phase. The convention
is to normalize the phase output from -180 degrees to +180 degrees. A phase
of -181 degrees is the same as a phase of +179 degrees.Below is an example
to illustrate how HSPICE wraps the phase.
Examples
Default Method (Without)
Freq Phase
3.16228k --> -167.7243
3.98107k --> 178.7844
If you use .OPTION UNWRAP = 1
3.16228k --> -167.7243
3.98107k --> -181.2156
If the phase value goes beyond -180, then it wraps to a positive value. At the
frequency 3.98107kHz the actual value is -181.2156, but by default, it is
wrapped to +178.7844.
HSPICE does the following calculation to wrap the phase:
-181.2156
+180.0000
----------1.2156
+180.0000
-1.2156
---------178.7844
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
709
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION VAMODEL
.OPTION VAMODEL
Specifies that name is the cell name that uses a Verilog-A definition rather than
the subcircuit definition when both exist (for use in HSPICE with Verilog-A).
Syntax
.OPTION VAMODEL [=name]
Description
Use this option to specify that name is the cell name that uses a Verilog-A
definition rather than the subcircuit definition when both exist. Each VAMODEL
option can take no more than one name. Multiple names need multiple
VAMODEL options.
If a name is not provided for the VAMODEL option, HSPICE uses the Verilog-A
definition whenever it is available. The VAMODEL option works on cell-based
instances only. Instance-based overriding is not allowed.
Examples
The following example specifies a Verilog-A definition for all instantiations of the
cell vco.
Example 1
.option vamodel=vco
Example 2 specifies a Verilog-A definition for all instantiations of the vco and
chargepump cells.
Example 2
.option vamodel=vco vamodel=chargepump
The following example instructs HSPICE to always use the Verilog-A definition
whenever it is available.
Example 3
.option vamodel
710
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION VERIFY
.OPTION VERIFY
Duplicates the LIST option.
Syntax
.OPTION VERIFY=[0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option as an alias for the LIST option.
See Also
.OPTION LIST
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
711
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION VFLOOR
.OPTION VFLOOR
Sets the minimum voltage to print in the output listing.
Syntax
.OPTION VFLOOR=x
Description
Use this option to set the minimum voltage to print in the output listing. All
voltages lower than VFLOOR print as 0. Affects only the output listing; VNTOL
(ABSV) sets the minimum voltage to use in a simulation.
See Also
.OPTION ABSV
.OPTION VNTOL
712
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION VNTOL
.OPTION VNTOL
Duplicates the ABSV option.
Syntax
.OPTION VNTOL=x
Default 5e-05
Description
Use this option as an alias for the ABSV option. Min value: 0; Max value: 10.
See Also
.OPTION ABSV
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
713
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WACC
.OPTION WACC
Activates the dynamic step control algorithm for a W-element transient
analysis.
Syntax
.OPTION WACC=x
Default -1 (variable, see below)
Description
Use this option to activate the dynamic step control algorithm for a W-element
transient analysis. WACC is a non-negative real value that can be set between
0.0 and 10.0. The WACC value influences a series of tolerances for W-element
simulation. The default value of WACC is determined by HSPICE, according to
the transmission line properties, such as loss and delay. Therefore, for different
transmission line, the default WACC value is different. It is suggested that you
not give a WACC value in the .option line, because it will give a constant value
to all the transmission lines in the netlist.HSPICE assigns WACC -1 if you do
not set a WACC option, or if you set .OPTION WACC. When a value of 1 is
specified, HSPICE assigns WACC a positive value. If a non-negative value is set
in the .option line (.OPTION WACC=XXX), HSPICE uses the specified WACC
value for all the W-elements. When WACC=0, HSPICE uses static breakpoint
with the interval between each two as the transmission line system delay.
Otherwise, when a positive value is set, W element uses dynamic time step
control, which may improve the performance, especially for short delay cases.
A large WACC value results in loose tolerance and bigger time steps, while small
values result in tight tolerances and smaller time steps.
The following refers to HSPICE only: For cases containing IBIS, PKG, EBD, or
ICM blocks, HSPICE turns WACC off automatically. If you want to use the
dynamic time step control algorithm for IBIS-related cases, you must set it
explicitly in the netlist. For example:
.option WACC $ Make HSPICE use automatically generated
WACC value for each W element
or
.option WACC=value
elements
$ Use this value for all the W
See Also
Using Dynamic Time-Step Control in the HSPICE User Guide: Signal
Integrity.
714
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WARN
.OPTION WARN
Enables or turns off SOA voltage warning message.
Syntax
.OPTION WARN=1|0
Default 1 or unspecified
Argument
Description
1 or
unspecified
Turns on the warning message
0
Turns off the warning message
Description
Use this option to enable or disable HSPICE warning messages when terminal
voltages of a device (MOSFET, BJT, Diode, Resistor, Capacitor, etc…) exceed
safe operating area (SOA).
The warning message is as follows:
**warning**(filename:line number): node_voltage_name =val
has exceeded node_voltage_name max =val
Control the number of warnings issued by using .OPTION MAXWARNS=n
See Also
.OPTION MAXWARNS
Safe Operating Area (SOA) Warnings
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
715
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WARN_SEP
.OPTION WARN_SEP
Separates out warnings to a file, while suppressing them in the *.lis file.
Syntax
.OPTION WARN_SEP [0|1]
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Setting a value of 1 for this option separates error and warning messages from
the *.lis file into a separate file (.warnlog). This file reports error and warning
message subheadings, contents, and summaries. This option also prints
message types to the terminal.
See Also
.OPTION WARNLIMIT (or) .OPTION WARNLIM
.OPTION LIS_NEW
716
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WARNLIMIT (or) .OPTION WARNLIM
.OPTION WARNLIMIT (or) .OPTION WARNLIM
Limits how many times certain warnings appear in the output listing.
Syntax
.OPTION WARNLIMIT=n
Description
Use this option to limit how many times the same warning appears in the output
listing. This reduces the output listing file size. The n parameter specifies the
maximum number of warnings for each warning type.
This limit applies to the following warning messages:
■
MOSFET has negative conductance.
■
Node conductance is zero.
■
Saturation current is too small.
■
Inductance or capacitance is too large.
See Also
.OPTION NOWARN
.OPTION MESSAGE_LIMIT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
717
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WAVE_POP
.OPTION WAVE_POP
Enables setting of buffer flush interval for .tr0 and .wdf files (HSPICE only).
Syntax
.OPTION WAVE_POP=val
Default 0.1 (10%)
Description
Sets waveform buffer flush interval as a percentage of the total simulation time.
The value can be set from 0.001 to 1, where 0.001 is 1% and 1 is 100% of the
total transient run time. .OPTION WAVE_POP values can also work when
.OPTION PSF is set. If the option is not set, then the waveform buffer will be
flushed at every 10% of the total simulation time.
Examples
In this example, the waveform buffer is flushed at every 5% of the total
simulation time.
.OPTION WAVE_POP=0.05
718
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WDELAYOPT
.OPTION WDELAYOPT
Globally applies the DELAYOPT keyword to a W-element transient analysis.
Syntax
.OPTION WDELAYOPT=[0|1|2|3]
Default
0
Description
Use this option as a global option which applies to all W-elements in a netlist.
.OPTION WDELAYOPT can be overridden by the DELAYOPT keyword for a
specified W-element.
■
In cases where WDELAYOPT is set in the .OPTION and the DELAYOPT
keyword is not specially set for Wxxx, the WDELAYOPT keyword is auto-set
for Wxxx.
■
In cases where the DELAYOPT keyword is already set for Wxxx, .OPTION
WDELAYOPT is overridden for the Wxxx.
■
In cases where neither .OPTION WDELAYOPT nor the DELAYOPT keyword
is set, the DELAYOPT keyword defaults to 0.
.OPTION WDELAYOPT helps construct a W-element transient (recursive
convolution) model with a higher level of accuracy. By specifying this option,
you can add the DELAYOPT keyword to the W-element instance line.
You can use DELAYOPT=0|1|2 to deactivate, activate, and automatically
determine, respectively.
Use DELAYOPT=3 to achieve a level of accuracy up to a tens of GHz operation
and involve harmonics up to THz order. With this option, line length limits are
removed, which frees the simulation from segmenting and allows
independence in the behavior of the RISETIME option setting. A setting of
WDELAYOPT=3 automatically detects whether or not frequency-dependent
phenomena need to be recorded, which makes it identical to the DELAYOPT=0
setting if it produces a high enough accuracy.
See Use DELAYOPT Keyword for Higher Frequency Ranges in the HSPICE
User Guide: Signal Integrity
See Also
.OPTION WINCLUDEGDIMAG
.OPTION RISETIME (or) .OPTION RISETI
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
719
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WDF
.OPTION WDF
Enables HSPICE to produce waveform files in WDF format.
Syntax
.OPTION WDF=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to enable HSPICE to produce waveform files in WDF format.
The WDF (Waveform Data File) format is a proprietary waveform storage
format. The WDF format compresses analog and logic waveform data, and
facilitates fast waveform access for large data files. The compression scheme
can be lossy or lossless (default). Use this option with the .PRINT or .PROBE
command.
■
.option WDF=0—Disables this option
■
.option WDF or .option WDF=1—Enables HSPICE to produce the
waveform file in WDF format
For the WDF waveform file, HSPICE automatically appends _wdf into the
output file root name to specify that it is in WDF format. The file names appear
as: *_wdf.tr#, *_wdf.sw#, or *_wdf.ac#.
For example, the WDF waveform output file will be named: design_wdf.tr0.
The WDF format is available to HSPICE RF for .AC, .DC, and .TRAN
analyses.
When the netlist contains .option wdf=1 and a .tran analysis statement
(with no .op statement in the netlist file), HSPICE creates the following output
files. See examples below.
720
■
.op0 — dc node voltage and dc operating points.
■
.op1 — transient voltage and transient operating points for the transient end
time.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WDF
Examples
Example 1
In this example, HSPICE creates these output files:
input_wdf.op0
[email protected]@spweep_index
.option WDF=1 opfile=1 split_dp=1
.tran '1n' '2n' start='0' sweep monte=10 firstrun=1
.op All 0.5n 1n 1.5n
Example 2
In this example, HSPICE outputs:
[email protected]@sweep_index
[email protected]@spweep_index
.option WDF=1 opfile=1 split_dp=2
See Also
.PRINT
.PROBE
.OPTION OPFILE
.OPTION SPLIT_DP
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
721
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WINCLUDEGDIMAG
.OPTION WINCLUDEGDIMAG
Globally activates the complex dielectric loss model in W-element analysis.
Syntax
.OPTION WINCLUDEGIMAG=[YES|NO]
Default
NO
Description
Use this option as a global option to activate the complex dielectric loss model
for all W-elements a netlist by introducing an imaginary term of the skin effect to
be considered. If WINCLUDEGDIMAG=YESand there is no wp input, the Welement regards the Gd matrix as the conventional model and then
automatically extracts constants for the complex dielectric model.
The .OPTION WINCLUDEGIMAG operates with the .OPTION WDELAYOPT
option.
■
In cases where WINCLUDEGDIMAG is set in the .OPTION and the
INCLUDEGDIMAG keyword is not specially set for Wxxx, the
INCLUDEGDIMAG is auto-set for Wxxx.
■
In cases where the INCLUDEGDIMAG keyword is already set for Wxxx,
.OPTION WINCLUDEGDIMAG is overridden for the Wxxx.
■
In cases where neither .OPTION WINCLUDEGDIMAG nor the
INCLUDEGDIMAG keyword is set, the INCLUDEGDIMAG keyword defaults to
N0.
For details about the INCLUDEGDIMAG keyword, see Fitting Procedure
Triggered by INCLUDEGDIMAG Keyword in the HSPICE USER GUIDE: Signal
Integrity.
See Also
.OPTION WDELAYOPT
.OPTION RISETIME (or) .OPTION RISETI
722
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WL
.OPTION WL
Reverses the order of the VSIZE MOS element.
Syntax
.OPTION WL=0|1
Default Value if option is not specified in the netlist: 0 Value if option name is
specified without a corresponding value: 1
Description
Use this option to reverse the order of the MOS element VSIZE. The default
order is length-width; this option changes the order to width-length.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
723
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION WNFLAG
.OPTION WNFLAG
Controls whether bin is selected based on w or w/nf.
Syntax
.OPTION WNFLAG=[0|1]
Description
Use this option to control whether HSPICE selects the bin based on the total
device width (WNFLAG=0) or based on the width of one finger of a multi fingered
device (WNFLAG=1).
For devices which are using a BSIM4 model, an element parameter
wnflag=[0|1] can be set, with the same effect as the option, and this
element parameter overrides then the option setting on an element basis.
Examples
For All Levels:
.option wnflag
M1 out in vdd vdd pmos w=10u l=1u nf=5
For BSIM4 models only:
M1 out in vdd vdd pmos w=10u l=1u nf=5 wnflag=1
724
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION XDTEMP
.OPTION XDTEMP
Defines how HSPICE interprets the DTEMP parameter.
Syntax
.OPTION XDTEMP=0|1
Default Value if option is not specified in the netlist: 0 (user-defined
parameter) Value if option name is specified without a corresponding value: 1
Description
Use this option to define how HSPICE interprets the DTEMP parameter, where
value is either:
■
0: Indicates a user-defined parameter
■
1: Indicates a temperature difference parameter
If you set .OPTION XDTEMP to 1, HSPICE adds the DTEMP value in the
subcircuit call command to all elements within the subcircuit that use the
DTEMP keyword syntax. The DTEMP parameter is cumulative throughout the
design hierarchy.
Examples
.OPTION XDTEMP
X1 2 0 SUB1 DTEMP=2
.SUBCKT SUB1 A B
R1 A B 1K DTEMP=3
C1 A B 1P
X2 A B sub2 DTEMP=4
.ENDS
.SUBCKT SUB2 A B
R2 A B 1K
.ENDS
In this example:
■
X1 sets a temperature difference (2 degrees Celsius) between the elements
within the subcircuit SUB1.
■
X2 (a subcircuit instance of X1) sets a temperature difference by the DTEMP
value of both X1 and X2 (2+4=6 degrees Celsius) between the elements
within the SUB2 subcircuit. The DTEMP value of each element in this
example is:
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
725
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION XDTEMP
Elements DTEMP Value (Celsius)
X1 2
X1.R1 2+3 =5
X1.C1 2
X2 2+4=6
X2.R2 6
726
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION (X0R,X0I)
.OPTION (X0R,X0I)
The first of three complex starting-trial points in the Muller algorithm used in
Pole/Zero analysis.
Syntax
.OPTION (X0R,X0I)= x,x
Default
X0R=-1.23456e6
X0I=0.0
Description
Use this option in Pole/Zero analysis if you need to change scale factors and
modify the initial Muller points, (X0R, X0I), (X1R, X1I) and (X2R, X2I). HSPICE
multiplies these initial points, and FMAX, by FSCAL.
Scale factors must satisfy the following relations: GSCAL = CSCAL ⋅ FSCAL
1
GSCAL = --------------------------------------------LSCAL ⋅ FSCAL
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION ITLPZ
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.PZ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
727
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION (X1R,X1I)
.OPTION (X1R,X1I)
The second of three complex starting-trial points in the Muller algorithm used in
Pole/Zero analysis.
Syntax
.OPTION (X1R,X1I)= x,x
Default X1R=1.23456e5 X1I=0.0
Description
Use this option in Pole/Zero analysis if you need to change scale factors and
modify the initial Muller points, (X0R, X0I), (X1R, X1I) and (X2R, X2I). HSPICE
multiplies these initial points, and FMAX, by FSCAL.
Scale factors must satisfy the following relations:
GSCAL = CSCAL ⋅ FSCAL
1
GSCAL = --------------------------------------------LSCAL ⋅ FSCAL
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION ITLPZ
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.PZ
728
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.OPTION (X2R,X21)
.OPTION (X2R,X21)
The third of three complex starting-trial points in the Muller algorithm used in
Pole/Zero analysis.
Syntax
.OPTION (X2R,X2I)= x,x
Default
X2R=+1.23456e6 X2I=0.0
Description
Use this option in Pole/Zero analysis if you need to change scale factors and
modify the initial Muller points, (X0R, X0I), (X1R, X1I) and (X2R, X2I). HSPICE
multiplies these initial points, and FMAX, by FSCAL.
Scale factors must satisfy the following relations: GSCAL = CSCAL ⋅ FSCAL
1
GSCAL = --------------------------------------------LSCAL ⋅ FSCAL
See Also
.OPTION CSCAL
.OPTION FMAX
.OPTION FSCAL
.OPTION GSCAL
.OPTION ITLPZ
.OPTION LSCAL
.OPTION PZABS
.OPTION PZTOL
.PZ
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
729
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.VARIATION Block Control Options
.VARIATION Block Control Options
The following options can be applied when doing .VARIATION analysis. Note
that no leading period is allowed with Variation Block control options.
Syntax
Option
Option
Option
Option
Option
Option
Option
Option
Option
Option
Normal_Limit=[1|2|3|4]
Ignore_Variation_Block=Yes
Ignore_Local_Variation=Yes
Ignore_Global_Variation=Yes
Ignore_Spatial_Variation=Yes
Ignore_Interconnect_Variation=Yes
Output_Sigma_Value=Value
Vary_Only Subckts=SubcktList
Do_Not_Vary Subckts=SubcktList
Add_Variation=Yes
Monte Carlo-Specific Options Using the Variation Block
Option
Option
Option
Option
Option
Option
Option
Random_Generator = [Default | MSG]
Stream =[x | Random | Default]
Use_Agauss_Format = Yes|No (Default: Yes)
Normal_Limit=Value
Output_Sigma_Value=Value
Print_Only Subckts=SubcktList
Do_Not_Print Subckts=SubcktList
Description
The following describes the available options:
■
Option Use_Agauss_Format=Yes Allows use of Gaussian sampling
methods as well as advanced sampling formats in a Variation Block.
■
Option Normal_Limit=[1|2|3|4] Limits the range of the Normal
distributions. This option allows a foundry to limit the perturbations to
parameter ranges where a model is still valid.
Where:
730
•
1: Infinity
•
2: Specifies no sampling value > 5 within 1000000 index
•
3: If a negative value is set it is automatically reset to 4
•
4: (Default) Numbers in the range +/- 4 σ are generated. The range
allowed is 0.1 to 20.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.VARIATION Block Control Options
■
Option Ignore_Variation_Block=Yes Ignores the Variation Block
and executes earlier style variations (traditional Monte Carlo analysis). By
default, the contents of the variation block are executed and other definitions
(AGAUSS, GAUSS, AUNIF, UNIF, LOT, and DEV) are ignored. Previous
methods of specifying variations on parameters and models are not
compatible with the Variation Block. By default, the contents of the Variation
Block are used and all other specifications are ignored. Thus no changes
are required in existing netlists other than adding the Variation Block.
■
Option Ignore_Local_Variation=Yes Excludes effects of local
variations in simulation. Default is No.
■
Option Ignore_Global_Variation=Yes Excludes effects of global
variations in simulation. Default is No.
■
Option Ignore_Spatial_Variation=Yes Excludes effects of spatial
variations in simulation. Default is No.
■
Option Ignore_Interconnect_Variation=Yes Excludes effects of
interconnect variations in simulation. Default is No. (See Interconnect
Variation in Star-RC with the HSPICE Flow.)
■
Option Output_Sigma_Value=Value Use to specify the sigma value of
the results of Monte Carlo, DCMatch, and ACMatch analyses. Default is 1,
range is 1 to 10. Note that this option only changes the output listings and
that the input sigma is not affected.
■
Option Vary_Only Subckts=SubcktList Use either this option to
limit variation to the specified subcircuits or the one below, but not both.
Actual subcircuit names are specified here (not the hierarchical names).
■
Option Do_Not_Vary Subckts=SubcktList Excludes variation on
the specified subcircuits. Use either this option to limit variation to the
specified subcircuits or the one above, but not both. Actual subcircuit names
are specified here (not the hierarchical names).
■
Option Screening_Method = Pearson|Spearman HSPICE
calculates the variables screened by importance using the Pearson or
Spearman algorithm. Default: Pearson.
See Also
Analyzing Variability and Using the Variation Block
Monte Carlo Analysis Using the Variation Block Flow
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
731
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.DESIGN_EXPLORATION Block Control Options
.DESIGN_EXPLORATION Block Control Options
The following options can be applied when doing .DESIGN_EXPLORATION
analysis. Note that no leading period is allowed with variation control options:
Syntax
Option
Option
Option
Option
Option
Option
Explore_only Subckts= SubcktList
Do_not_explore Subckts= SubcktList
Export=yes|no
Exploration_method=external Block_name=Block_name
Ignore_exploration= yes|no
Secondary_param= yes|no
Description
The Design Exploration control options are described below:
732
■
Option Explore_only Subckts= SubcktList This command is
executed hierarchically—the specified subcircuits and all instantiated
subcircuits and elements underneath are affected. Thus, if an inverter with
name INV1 is placed in a digital control block called DIGITAL and in an
analog block ANALOG, and OptionExplore_only Subckts = ANALOG,
then the perturbations only affect the INV1 in the analog block. You must
create a new inverter, INV1analog, with the new device sizes.
■
Option Do_not_explore Subckts= SubcktList Excludes listed
subcircuits.
■
Option Export=yes|no If yes, exports extraction data and runs one
simulation with the original netlist. If no (default), runs a simulation with
Exploration data.
■
Option Exploration_method=external
Block_name=Block_name The Block_name is the same as the name
specified in the .DATA block; HSPICE will sweep the row content with the
EXCommandexplore.
■
Option Ignore_exploration= yes|no (Default=no) HSPICE ignores
the content in the design_exploration block, when
Ignore_exploration=yes.
■
Option Secondary_param= yes|no (Default=no) If
Secondary_param=yes, HSPICE exports the MOSFET secondary
instance parameters to a *.mex file (created when option export=yes),
and also permits the secondary parameters to be imported as a column
header in the .DATA block (option export=no).
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.DESIGN_EXPLORATION Block Control Options
See Also
.DESIGN_EXPLORATION
Exploration Block
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
733
Chapter 3: HSPICE and RF Netlist Simulation Control Options
.DESIGN_EXPLORATION Block Control Options
734
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
4
4
Digital Vector File Commands
Contains an alphabetical listing of the commands you can use in a digital vector
file.
You can use the following HSPICE/HSPICE RF commands in a digital vector
file.
ENABLE
SLOPE
VIH
IDELAY
TDELAY
VIL
IO
TFALL
VNAME
ODELAY
TRISE
VOH
OUT or OUTZ
TRIZ
VOL
PERIOD
TSKIP
VREF
RADIX
TUNIT
VTH
For additional information on vector file usage, see Specifying a Digital Vector
File and Mixed Mode Stimuli in the HSPICE User Guide: Simulation and
Analysis.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
735
Chapter 4: Digital Vector File Commands
ENABLE
ENABLE
Specifies the controlling signal(s) for bidirectional signals.
Syntax
ENABLE controlling_signalname mask
ArgumentArgument
DescriptionDescription
controlling_signalname
Controlling signal for bidirectional signals. Must be an input
signal with a radix of 1. The bidirectional signals become
output when the controlling signal is at state 1 (or high). To
reverse this default control logic, start the control signal
name with a tilde (~).
mask
Defines the bidirectional signals to which ENABLE applies.
Description
Use this command to specify the controlling signal(s) for bidirectional signals.
All bidirectional signals require an ENABLE command. If you specify more than
one ENABLE command, the last command overrides the previous command
and HSPICE issues a warning message:
[Warning]:[line 6] resetting enable signal to WENB for
bit ’XYZ’
Examples
radix 144
io ibb
vname a x[[3:0]] y[[3:0]]
enable a 0 F 0
enable ~a 0 0 F
In this example, the x and y signals are bidirectional as defined by the b in the
io line.
736
■
The first enable command indicates that x (as defined by the position of F)
becomes output when the a signal is 1.
■
The second enable specifies that the y bidirectional bus becomes output
when the a signal is 0.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
IDELAY
IDELAY
Defines an input delay time for bidirectional signals.
Syntax
IDELAY delay_value [mask]
Argument
Description
delay_value
Time delay to apply to the signals.
mask
Signals to which the delay applies. If you do not provide a mask value,
the delay value applies to all signals.
Description
Use this command to define an input delay time for bidirectional signals relative
to the absolute time of each row in the Tabular Data section. HSPICE ignores
IDELAY settings on output signals and issues a warning message.
You can specify more than one TDELAY, IDELAY, or ODELAY command.
■
If you apply more than one TDELAY (IDELAY, ODELAY) command to a
signal, the last command overrides the previous commands and HSPICE or
HSPICE RF issues a warning.
■
If you do not specify the signal delays in a TDELAY, IDELAY, or ODELAY
command, HSPICE or HSPICE RF defaults to zero.
Examples
RADIX 1 1 4 1234 11111111
IO i i o iiib iiiiiiii
VNAME V1 V2 VX[[3:0]] V4 V5[[1:0]] V6[[0:2]] V7[[0:3]]
+ V8 V9 V10 V11 V12 V13 V14 V15
TDELAY 1.0
TDELAY -1.2 0 1 F 0000 00000000
TDELAY 1.5 0 0 0 1370 00000000
IDELAY 2.0 0 0 0 000F 00000000
ODELAY 3.0 0 0 0 000F 00000000
This example does not specify the TUNIT command so HSPICE or HSPICE RF
uses the default, ns, as the time unit for this example. The first TDELAY
command indicates that all signals have the same delay time of 1.0ns.
Subsequent TDELAY, IDELAY, or ODELAY commands overrule the delay time
of some signals.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
737
Chapter 4: Digital Vector File Commands
IDELAY
■
The delay time for the V2 and Vx signals is -1.2.
■
The delay time for the V4, V5[0:1], and V6[0:2] signals is 1.5.
■
The input delay time for the V7[0:3] signals is 2.0, and the output delay time
is 3.0.
See Also
ODELAY
TDELAY
TUNIT
738
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
IO
IO
Defines the type for each vector: input, bidirectional, output, or unused.
Syntax
IO I | O | B | U
[I | O | B | U ...]
Argument
Description
i
Input that HSPICE uses to stimulate the circuit.
o
Expected output that HSPICE compares with the simulated outputs.
b
Bidirectional vector.
u
Unused vector that HSPICE ignores.
Description
Use this command to define the type for each vector. The line starts with the IO
keyword followed by a string of i, b, o, or u definitions. These definitions indicate
whether each corresponding vector is an input (i), bidirectional (b), output (o),
or unused (u) vector.
■
If you do not specify the IO command, HSPICE or HSPICE RF assumes
that all signals are input signals.
■
If you define more than one IO command, the last command overrides
previous commands.
Examples
io i i i bbbb iiiioouu
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
739
Chapter 4: Digital Vector File Commands
ODELAY
ODELAY
Defines an output delay time for bidirectional signals.
Syntax
ODELAY delay_value [mask]
Argument
Description
delay_value
Time delay to apply to the signals.
mask
Signals to which the delay applies. If you do not provide a mask
value, the delay value applies to all signals.
Description
Use this command to define an output delay time for bidirectional signals
relative to the absolute time of each row in the Tabular Data section.
HSPICE ignores ODELAY settings on input signals and issues a warning
message.
You can specify more than one TDELAY, IDELAY, or ODELAY command.
■
If you apply more than one TDELAY (IDELAY, ODELAY) command to a
signal, the last command overrides the previous commands and HSPICE
issues a warning.
■
If you do not specify the signal delays in a TDELAY, IDELAY, or ODELAY
command, HSPICE defaults to zero.
Examples
RADIX 1 1 4 1234 11111111
IO i i o iiib iiiiiiii
VNAME V1 V2 VX[[3:0]] V4 V5[[1:0]] V6[[0:2]] V7[[0:3]]
+ V8 V9 V10 V11 V12 V13 V14 V15
TDELAY 1.0
TDELAY -1.2 0 1 F 0000 00000000
TDELAY 1.5 0 0 0 1370 00000000
IDELAY 2.0 0 0 0 000F 00000000
ODELAY 3.0 0 0 0 000F 00000000
This example does not specify the TUNIT command so HSPICE or HSPICE RF
uses the default, ns, as the time unit for this example. The first TDELAY
command indicates that all signals have the same delay time of 1.0ns.
740
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
ODELAY
Subsequent TDELAY, IDELAY, or ODELAY commands overrule the delay time
of some signals.
■
The delay time for the V2 and Vx signals is -1.2.
■
The delay time for the V4, V5[0:1], and V6[0:2] signals is 1.5.
■
The input delay time for the V7[0:3] signals is 2.0 and the output delay time
is 3.0.
See Also
IDELAY
TDELAY
TUNIT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
741
Chapter 4: Digital Vector File Commands
OUT or OUTZ
OUT or OUTZ
Specifies output resistance for each signal for which the mask applies. OUT and
OUTZ are equivalent.
Syntax
OUT output_resistance [mask]
Argument
Description
output_resistance
Output resistance for an input signal. The default is 0.
mask
Signals to which the output resistance applies. If you do not
provide a mask value, the output resistance value applies to all
input signals.
Description
The OUT and OUTZ keywords are equivalent: use these commands to specify
output resistance for each signal (for which the mask applies). OUT or OUTZ
applies to input signals only.
■
If you do not specify the output resistance of a signal in an OUT (or OUTZ)
command, HSPICE uses the default (zero).
■
If you specify more than one OUT (or OUTZ) command for a signal, the last
command overrides the previous commands and HSPICE issues a warning
message.
The OUT (or OUTZ) commands have no effect on the expected output signals.
Examples
OUT 15.1
OUT 150 1 1 1 0000 00000000
OUTZ 50.5 0 0 0 137F 00000000
The first OUT command in this example creates a 15.1 ohm resistor to place in
series with all vector inputs. The next OUT command sets the resistance to 150
ohms for vectors 1 to 3. The OUTZ command changes the resistance to 50.5
ohms for vectors 4 through 7.
742
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
PERIOD
PERIOD
Defines the time interval for the Tabular Data section.
Syntax
PERIOD time_interval
Argument
Description
time_interval
Time interval for the Tabular Data.
Description
Use this command to define the time interval for the Tabular Data section. You
do not need to specify the absolute time at every time point. If you use a
PERIOD command without the TSKIP command, the Tabular Data section
contains only signal values, not absolute times. The TUNIT command defines
the time unit of the PERIOD.
Examples
radix 1111 1111
period 10
1000 1000
1100 1100
1010 1001
■
The first row of the tabular data (1000 1000) is at time 0ns.
■
The second row (1100 1100) is at 10ns.
■
The third row (1010 1001) is at 20ns.
See Also
TSKIP
TUNIT
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
743
Chapter 4: Digital Vector File Commands
RADIX
RADIX
Specifies the number of bits associated with each vector.
Syntax
RADIX number_of_bits [number_of_bits...]
Argument
Description
number_of_bits
Specifies the number of bits in one vector in the digital vector
file. You must include a separate number_of_bits argument in
the RADIX command for each vector listed in the file.
Description
Use this command to specify the number of bits associated with each vector.
Valid values for the number of bits range from 1 to 4.
A digital vector file must contain only one RADIX command and it must be the
first non-comment line in the file.
Table 2
Valid Values for the RADIX command
# bits
Radix
Number System
Valid Digits
1
2
Binary
0, 1
2
4
–
0–3
3
8
Octal
0–7
4
16
Hexadecimal
0–F
Examples
; start of Vector Pattern Definition section
RADIX 1 1 4 1234 1111 1111
VNAME A B C[[3:0]] I9 I[[8:7]] I[[6:4]] I[[3:0]] O7 O6 O5 O4
+ O3 O2 O1 O0
IO I I I IIII OOOO OOOO
This example illustrates two 1-bit signals followed by a 4-bit signal, followed by
one each 1-bit, 2-bit, 3-bit, and 4-bit signals, and finally eight 1-bit signals.
744
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
SLOPE
SLOPE
Specifies the rise/fall time for the input signal.
Syntax
SLOPE [input_rise_time | input_fall_time] [mask]
Argument
Description
input_rise_time
Rise time of the input signal.
input_fall_time
Fall time of the input signal.
mask
Name of a signal to which the SLOPE command applies. If you
do not specify a mask value, the SLOPE command applies to
all signals.
Description
Use this command to specify the rise/fall time for the input signal. Use the
TUNIT command to define the time unit for this command.
■
If you do not specify the SLOPE command, the default slope value is 0.1 ns.
■
If you specify more than one SLOPE command, the last command overrides
the previous commands and HSPICE or HSPICE RF issues a warning
message.
The SLOPE command has no effect on the expected output signals. You can
specify the optional TRISE and TFALL commands to overrule the rise time and
fall time of a signal.
Examples
In the following example, the rising and falling times of all signals are 1.2 ns.
Example 1
SLOPE 1.2
In the following example, the rising/falling time is 1.1 ns for the first, second,
sixth, and seventh signals.
Example 2
SLOPE 1.1 1100 0110
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
745
Chapter 4: Digital Vector File Commands
SLOPE
See Also
TFALL
TRISE
TUNIT
746
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
TDELAY
TDELAY
Defines the delay time for both input and output signals in the Tabular Data
section.
Syntax
TDELAY delay_value [mask]
Argument
Description
delay_value
Time delay to apply to the signals.
mask
Signals to which the delay applies. If you do not provide a mask
value, the delay value applies to all signals.
Description
Use this command to define the delay time of both input and output signals
relative to the absolute time of each row in the Tabular Data section.
You can specify more than one TDELAY, IDELAY, or ODELAY command.
■
If you apply more than one TDELAY (IDELAY, ODELAY) command to a
signal, the last command overrides the previous commands and HSPICE or
HSPICE RF issues a warning.
■
If you do not specify the signal delays in a TDELAY, IDELAY, or ODELAY
command, HSPICE or HSPICE RF defaults to zero.
Examples
RADIX 1 1 4 1234 11111111
IO i i o iiib iiiiiiii
VNAME V1 V2 VX[[3:0]] V4 V5[[1:0]] V6[[0:2]] V7[[0:3]]
+ V8 V9 V10 V11 V12 V13 V14 V15
TDELAY 1.0
TDELAY -1.2 0 1 F 0000 00000000
TDELAY 1.5 0 0 0 1370 00000000
IDELAY 2.0 0 0 0 000F 00000000
ODELAY 3.0 0 0 0 000F 00000000
This example does not specify the TUNIT command so HSPICE or HSPICE RF
uses the default, ns, as the time unit for this example. The first TDELAY
command indicates that all signals have the same delay time of 1.0ns.
Subsequent TDELAY, IDELAY, or ODELAY commands overrule the delay time
of some signals.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
747
Chapter 4: Digital Vector File Commands
TDELAY
■
The delay time for the V2 and Vx signals is -1.2.
■
The delay time for the V4, V5[0:1], and V6[0:2] signals is 1.5.
■
The input delay time for the V7[0:3] signals is 2.0, and the output delay time
is 3.0.
See Also
IDELAY
ODELAY
TUNIT
748
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
TFALL
TFALL
Specifies the fall time of each input signal for which the mask applies.
Syntax
TFALL input_fall_time [mask]
Argument
Description
input_fall_time
Fall time of the input signal.
mask
Name of a signal to which the TFALL command applies. If you do not
specify a mask value, the TFALL command applies to all input
signals.
Description
Use this command to specify the fall time of each input signal for which the
mask applies. The TUNIT command defines the time unit of TFALL.
■
If you do not use any TFALL command to specify the fall time of the signals,
HSPICE or HSPICE RF uses the value defined in the slope command.
■
If you apply more than one TFALL command to a signal, the last command
overrides the previous commands and HSPICE or HSPICE RF issues a
warning message.
TFALL commands have no effect on the expected output signals.
Examples
In Example1, the TFALL command assigns a fall time of 0.5 time units to all
vectors.
Example 1
TFALL 0.5
In the following example, the TFALL command assigns a fall time of 0.3 time
units overriding the older setting of 0.5 to vectors 2, 3, and 4 to 7.
Example 2
TFALL 0.3 0 1 1 137F 00000000
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
749
Chapter 4: Digital Vector File Commands
TFALL
In the following example, the TFALL command assigns a fall time of 0.9 time
units to vectors 8 through 11.
TFALL 0.9 0 0 0 0000 11110000
See Also
TRISE
TUNIT
750
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
TRISE
TRISE
Specifies the rise time of each input signal for which the mask applies.
Syntax
TRISE input_rise_time [mask]
ArgumentArgument
DescriptionDescription
input_rise_time
Rise time of the input signal.
mask
Name of a signal to which the TRISE command applies. If you
do not specify a mask value, the TRISE command applies to all
input signals.
Description
Use this command to specify the rise time of each input signal for which the
mask applies. The TUNIT command defines the time unit of TRISE.
■
If you do not use any TRISE command to specify the rising time of the
signals, HSPICE or HSPICE RF uses the value defined in the slope
command.
■
If you apply more than one TRISE command to a signal, the last command
overrides the previous commands and HSPICE or HSPICE RF issues a
warning message.
TRISE commands have no effect on the expected output signals.
Examples
In this example, the TRISE command assigns a rise time of 0.3 time units to all
vectors.
Example 1
TRISE 0.3
In this example, the TRISE command assigns a rise time of 0.5 time units
overriding the older setting of 0.3 in at least some of the bits in vectors 2, 3, and
4 through 7.
Example 2
TRISE 0.5 0 1 1 137F 00000000
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
751
Chapter 4: Digital Vector File Commands
TRISE
In Example 3, the TRISE command assigns a rise time of 0.8 time units to
vectors 8 through 11.
Example 3
TRISE 0.8 0 0 0 0000 11110000
See Also
TFALL
TUNIT
752
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
TRIZ
TRIZ
Specifies the output impedance when the signal for which the mask applies is
in tristate.
Syntax
TRIZ output_impedance [mask]
Argument
Description
output_impedance
Output impedance of the input signal.
mask
Name of a signal to which the TRIZ command applies. If
you do not specify a mask value, the TRIZ command
applies to all input signals.
Description
Use this command to specify the output impedance when the signal (for which
the mask applies) is in tristate; TRIZ applies only to the input signals.
■
If you do not specify the tristate impedance of a signal, in a TRIZ command,
HSPICE or HSPICE RF assumes 1000M.
■
If you apply more than one TRIZ command to a signal, the last command
overrides the previous commands and HSPICE or HSPICE RF issues a
warning.
TRIZ commands have no effect on the expected output signals.
Examples
TRIZ 15.1Meg
TRIZ 150Meg 1 1 1 0000 00000000
TRIZ 50.5Meg 0 0 0 137F 00000000
■
The first TRIZ command sets the high impedance resistance globally at
15.1 Mohms.
■
The second TRIZ command increases the value to 150 Mohms for vectors
1 to 3.
■
The last TRIZ command increases the value to 50.5 Mohms for vectors 4
through 7.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
753
Chapter 4: Digital Vector File Commands
TSKIP
TSKIP
Causes HSPICE to ignore the absolute time field in the tabular data.
Syntax
TSKIP absolute_time tabular_data ...
Argument
Description
absolute_time
Absolute time.
tabular_data
Data captured at absolute_time.
Description
Use this command to cause HSPICE to ignore the absolute time field in the
tabular data. You can then keep, but ignore, the absolute time field for each row
in the tabular data when you use the .PERIOD command.
You might do this, for example, if for testing reasons the absolute times are not
perfectly periodic. Another reason might be that a path in the circuit does not
meet timing, but you might still use it as part of a test bench. Initially, HSPICE
writes to the vector file using absolute time. After you fix the circuit, you might
want to use periodic data.
Examples
radix 1111 1111
period 10
tskip
11.0 1000 1000
20.0 1100 1100
33.0 1010 1001
HSPICE or HSPICE RF ignores the absolute times 11.0, 20.0 and 33.0, but
HSPICE does process the tabular data on the same lines as those absolute
times.
See Also
PERIOD
754
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
TUNIT
TUNIT
Defines the time unit for PERIOD, TDELAY,IDELAY, ODELAY, SLOPE, TRISE,
TFALL, and absolute time.
Syntax
TUNIT [fs|ps|ns|us|ms]
Argument
Description
fs
femtosecond
ps
picosecond
ns
nanosecond (default)
us
microsecond
ms
millisecond
Description
Use this command to define the time unit in the digital vector file for PERIOD,
TDELAY, IDELAY, ODELAY, SLOPE, TRISE, TFALL, and absolute time.
■
If you do not specify the TUNIT command, the default time unit value is ns.
■
If you define more than one TUNIT command, the last command overrides
the previous command.
Examples
The TUNIT command in this example specifies that the absolute times in the
Tabular Data section are 11.0ns, 20.0ns, and 33.0ns.
TUNIT ns
11.0 1000 1000
20.0 1100 1100
33.0 1010 1001
The following are legal ways to write the time values.
tunit
tunit
tunit
tunit
tunit
999ns
.99ps
.99e+6ps
999 ns
.99 ps
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
755
Chapter 4: Digital Vector File Commands
TUNIT
The following are examples of wrong syntax which will result in an error
message:
tunit .99eps
tunit .99 e+6ps
tunit .99 eps
See Also
IDELAY
ODELAY
PERIOD
SLOPE
TDELAY
TFALL
TRISE
756
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
VIH
VIH
Specifies the logic-high voltage for each input signal to which the mask applies.
Syntax
VIH logic-high_voltage [mask]
Argument
Description
logic-high_voltage
Logic-high voltage for an input signal. The default is 3.3.
mask
Name of a signal to which the VIH command applies. If you
do not specify a mask value, the VIH command applies to all
input signals.
Description
Use this command to specify the logic-high voltage for each input signal to
which the mask applies.
■
If you do not specify the logic high voltage of the signals in a VIH command,
HSPICE assumes 3.3.
■
If you use more than one VIH command for a signal, the last command
overrides previous commands and HSPICE issues a warning.
VIH commands have no effect on the expected output signals.
Examples
VIH 5.0
VIH 3.5 0 0 0 0000 11111111
■
The first VIH command sets all input vectors to 5V when they are high.
■
The last VIH command changes the logic-high voltage from 5V to 3.5V for
the last eight vectors.
See Also
VIL
VOH
VOL
VTH
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
757
Chapter 4: Digital Vector File Commands
VIL
VIL
Specifies the logic-low voltage for each input signal to which the mask applies.
Syntax
VIL logic-low_voltage [mask]
ArgumentArgument
DescriptionDescription
logic-low_voltage
Logic-low voltage for an input signal. The default is 0.0.
mask
Name of a signal to which the VIL command applies. If you
do not specify a mask value, the VIL command applies to all
input signals.
Description
Use this command to specify the logic-low voltage for each input signal to
which the mask applies.
■
If you do not specify the logic-low voltage of the signals in a VIL command,
HSPICE or HSPICE RF assumes 0.0.
■
If you use more than one VIL command for a signal, the last command
overrides previous commands and HSPICE issues a warning.
VIL commands have no effect on the expected output signals.
Examples
VIL 0.0
VIL 0.5 0 0 0 0000 11111111
■
The first VIL command sets the logic-low voltage to 0V for all vectors.
■
The second VIL command changes the logic-low voltage to 0.5V for the last
eight vectors.
See Also
VIH
VOH
VOL
VTH
758
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
VNAME
VNAME
Defines the name of each vector.
Syntax
VNAME vector_name [[starting_index:ending_index]]
Argument
Description
vector_name
Name of the vector, or range of vectors.
starting_index
First bit in a range of vector names.
ending_index
Last bit in a range of vector names. You can associate a single name
with multiple bits (such as bus notation).
The opening and closing brackets and the colon are required; they
indicate that this is a range. The vector name must correlate with the
number of bits available.
You can nest the bus definition inside other grouping symbols, such
as { }, ( ), [ ], and so on. The bus indices expand in the specified order
Description
Use this command to define the name of each vector. If you do not specify
VNAME, HSPICE or HSPICE RF assigns a default name to each signal: V1, V2,
V3, and so on. If you define more than one VNAME command, the last
command overrides the previous command.
Examples
Auto-defined names for each signal.
Example 1
RADIX 1 1 1 1 1 1 1 1 1 1 1 1
VNAME V1 V2 V3 V4 V5 V6 V7 V8 V9 V10 V11 V12
Example 2 represents a0, a1, a2, and a3, in that order. HSPICE or HSPICE RF
does not reverse the order to make a3 the first bit. The bit order is MSB:LSB,
which means most significant bit to least significant bit. For example, you can
represent a 5-bit bus such as: {a4 a3 a2 a1 a0}, using this notation: a[[4:0]].
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
759
Chapter 4: Digital Vector File Commands
VNAME
The high bit is a4, which represents 24. It is the largest value and therefore is
the MSB.
Example 2
VNAME a[[0:3]]
HSPICE or HSPICE RF generates voltage sources with the following names:
VA0 VA1 VB4 VB3 VB2 VB1
■
VA0 and VB4 are the MSBs.
■
VA1 and VB1 are the LSBs.
Example 3
RADIX 2 4
VNAME VA[[0:1]] VB[[4:1]]
For Example 4, HSPICE or HSPICE RF generates voltage sources with the
following names: VA[0] VA[1] VB<4> VB<3> VB<2> VB<1>
Example 4
VNAME VA[[0:1]] VB<[4:1]>
Example 5 specifies a single bit of a bus. This range creates a voltage source
named VA [2].
Example 5
VNAME VA[[2:2]]
Example 6 generates signals named A0, A1, A2, ... A23.
Example 6
RADIX 444444
VNAME A[[0:23]]
760
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
VOH
VOH
Specifies the logic-high threshold voltage for each output signal to which the
mask applies.
Syntax
VOH logic-high_threshold_voltage [mask]
ArgumentArgument
DescriptionDescription
logic-high_threshold_voltage
Logic-high threshold voltage for an output vector. The
default is 2.66.
mask
Name of a signal to which the VOH command applies. If you
do not specify a mask value, the VOH command applies to
all output signals.
Description
Use this command to specify the logic-high threshold voltage for each output
signal to which the mask applies.
■
If you do not specify the logic-high threshold voltage in a VOH command,
HSPICE assumes 2.64.
■
If you apply more than one VOH command to a signal, the last command
overrides the previous commands and HSPICE issues a warning.
VOH commands have no effect on input signals.
Examples
VOH 4.75
VOH 4.5 1 1 1 137F 00000000
VOH 3.5 0 0 0 0000 11111111
■
The first line tries to set a logic-high threshold output voltage of 4.75V, but it
is redundant.
■
The second line changes the voltage level to 4.5V for the first seven vectors.
■
The last line changes the last eight vectors to a 3.5V logic-high threshold
output.
These second and third lines completely override the first VOH command.
If you do not define either VOH or VOL, HSPICE or HSPICE RF uses VTH
(default or defined).
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
761
Chapter 4: Digital Vector File Commands
VOH
See Also
VIH
VIL
VOL
VTH
762
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
VOL
VOL
Specifies the logic-low threshold voltage for each output signal to which the
mask applies.
Syntax
VOL logic-low_threshold_voltage [mask]
Argument
Description
logic-low_voltage
Logic-low threshold voltage for an output vector. The
default is 0.64.
mask
Name of a signal to which the VOL command applies.
If you do not specify a mask value, the VOL command
applies to all output signals.
Description
Use this command to specify the logic-low threshold voltage for each output
signal to which the mask applies.
■
If you do not specify the logic-low threshold voltage in a VOL command,
HSPICE assumes 0.66.
■
If you apply more than one VOL command to a signal, the last command
overrides the previous commands and HSPICE issues a warning.
Examples
VOL 0.0
VOL 0.2 0 0 0 137F 00000000
VOL 0.5 1 1 1 0000 00000000
■
The first VOL command sets the logic-low threshold output to 0V.
■
The second VOL command sets the output voltage to 0.2V for the fourth
through seventh vectors.
■
The last command increases the voltage further to 0.5V for the first three
vectors.
These second and third lines completely override the first VOL command.
If you do not define either VOH or VOL, HSPICE or HSPICE RF uses VTH
(default or defined).
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
763
Chapter 4: Digital Vector File Commands
VOL
See Also
VIH
VIL
VOH
VTH
764
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
VREF
VREF
Specifies the name of the reference voltage for each input vector to which the
mask applies.
Syntax
VREF reference_voltage
Argument
Description
reference_voltage
Reference voltage for each input vector. The default is 0.
Description
Use this command to specify the name of the reference voltage for each input
vector to which the mask applies. Similar to the TDELAY command, the VREF
command applies only to input signals.
■
If you do not specify the reference voltage name of the signals in a VREF
command, HSPICE assumes 0.
■
If you apply more than one VREF command, the last command overrides the
previous commands and HSPICE issues a warning.
VREF commands have no effect on the output signals.
Examples
VNAME v1 v2 v3 v4 v5[[1:0]] v6[[2:0]] v7[[0:3]] v8 v9 v10
VREF 0
VREF 0 111 137F 000
VREF vss 0 0 0 0000 111
When HSPICE or HSPICE RF implements these commands into the netlist, the
voltage source realizes v1:
v1 V1 0 pwl(......)
as well as v2, v3, v4, v5, v6, and v7.
However, v8 is realized by
V8 V8 vss pwl(......)
v9 and v10 use a syntax similar to v8.
See Also
TDELAY
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
765
Chapter 4: Digital Vector File Commands
VTH
VTH
Specifies the logic threshold voltage for each output signal to which the mask
applies.
Syntax
VTH logic-threshold_voltage
Argumentt
Description
logic-threshold_voltage
Logic-threshold voltage for an output vector. The
default is 1.65.
Description
Use this command to specify the logic threshold voltage for each output signal
to which the mask applies. It is similar to the TDELAY command. The threshold
voltage determines the logic state of output signals for comparison with the
expected output signals.
■
If you do not specify the threshold voltage of the signals in a VTH command,
HSPICE assumes 1.65.
■
If you apply more than one VTH command to a signal, the last command
overrides the previous commands and HSPICE or HSPICE RF issues a
warning.
VTH commands have no effect on the input signals.
Examples
VTH 1.75
VTH 2.5 1 1 1 137F 00000000
VTH 1.75 0 0 0 0000 11111111
■
The first VTH command sets the logic threshold voltage at 1.75V.
■
The next line changes that threshold to 2.5V for the first 7 vectors.
■
The last line changes that threshold to 1.75V for the last 8 vectors.
All of these examples apply the same vector pattern and both output and input
control commands, so the vectors are all bidirectional.
See Also
TDELAY
VIH
VIL
766
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Chapter 4: Digital Vector File Commands
VTH
VOH
VOL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
767
Chapter 4: Digital Vector File Commands
VTH
768
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
A
A
Obsolete Commands and Options
Describes the obsolete or rarely used HSPICE commands.
The following commands and options are included for completeness only. More
efficient functionality and commands are available.
■
.ACDCFACTOR
■
.GRAPH
■
.MODEL Command for .GRAPH
■
.NET
■
.PLOT
■
.WIDTH
■
.OPTION ALT999 or ALT9999
■
.OPTION BKPSIZ
■
.OPTION CDS
■
.OPTION CO
■
.DEGINFO
■
.OPTION H9007
■
.OPTION MEASSORT
■
.OPTION MENTOR
■
.OPTION MODSRH
■
.OPTION NOPAGE
■
.OPTION PIVREF
■
.OPTION PIVREL
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
769
Appendix A: Obsolete Commands and Options
.ACDCFACTOR
■
.OPTION PLIM
■
.OPTION SDA
■
.OPTION SIM_LA_MINMODE
■
.OPTION SPICE
■
.OPTION ZUKEN
.ACDCFACTOR
OBSOLETE with the D-2010.03 release. Invokes degradation characterization
under DC/AC stress, respectively.
Syntax
.ACDCFACTOR vds=value vgs=value [vbs=value] Time=value
Argument
Description
vds
vds value for the dc calculation
vgs
vgs value for the dc calculation
vbs
vbs value for the dc calculation
Time
Time to calculate the acdcfactor
Description
This command invokes degradation characterization under DC/AC stress,
respectively, based on the customized algorithm(s) implemented in the MOSRA
API model. A new output file *.acdcfactor is generated.
Example
.ACDCFACTOR Vds=1.0 Vgs=1.2 Vbs=0 time = 4n
770
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.GRAPH
.GRAPH
OBSOLETE. Provides high-resolution plots of HSPICE simulation results. This
is an obsolete command. You can gain the same functionality by using the
.PROBE command.
.GRAPH antype [MODEL=mname] unam1= ov1,
+ [unam2=ov2] ... [unamn=ovn] (plo,phi)
Argument
Description
antype
Type of analysis for the specified plots (outputs). Analysis types are:
DC, AC, TRAN, NOISE, or DISTO.
mname
Plot model name, referenced in the .GRAPH command. Use .GRAPH
and its plot name to create high-resolution plots directly from HSPICE.
unam1...
You can define output names, which correspond to the ov1 ov2 ...
output variables (unam1 unam2 ...), and use them as labels, instead of
output variables for a high resolution graphic output.
ov1 ...
Output variables to print. Can be voltage, current, or element template
variables from a different type of analysis. You can also use algebraic
expressions as output variables, but you must define them inside the
PAR( ) command.
plo, phi
Lower and upper plot limits. Set the plot limits only at the end of
the .GRAPH command.
Description
Use this command when you need high-resolution plots of HSPICE simulation
results.
Each .GRAPH command creates a new .gr# file, where # ranges first from 0 to
9 and then from a to z. You can create up to 10000 graph files.
You can include wildcards in .GRAPH commands.
You cannot use .GRAPH commands in the Windows version of HSPICE or in
HSPICE RF.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
771
Appendix A: Obsolete Commands and Options
.GRAPH
Example
.GRAPH DC cgb=lx18(m1) cgd=lx19(m1)
+ cgs=lx20(m1)
.GRAPH DC MODEL=plotbjt
+ model_ib=i2(q1) meas_ib=par(ib)
+ model_ic=i1(q1) meas_ic=par(ic)
+ model_beta=par('i1(q1)/i2(q1)')
+ meas_beta=par('par(ic)/par(ib)')(1e-10,1e-1)
.MODEL plotbjt PLOT MONO=1 YSCAL=2 XSCAL=2
+ XMIN=1e-8 XMAX=1e-1
772
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.MODEL Command for .GRAPH
.MODEL Command for .GRAPH
OBSOLETE. For a description of how to use the .MODEL command with
.GRAPH, see .MODEL.
Syntax
N/A
Argument
Description
MONO
Monotonic option. MONO=1 automatically resets the x-axis, if any
change occurs in the x direction. Default 0.0
TIC
Shows tick marks. Default 0.0
FREQ
Plots symbol frequency.Default 0.0
■
A value of 0 does not generate plot symbols.
A value of n generates a plot symbol every n points.
This is not the same as the FREQ keyword in element commands.
■
XGRID, YGRID
Set these values to 1.0, to turn on the axis grid lines. Default 0.0
XMIN, XMAX
■
If XMIN is not equal to XMAX, then XMIN and XMAX determine
the x-axis plot limits.
■
If XMIN equals XMAX, or if you do not set XMIN and XMAX,
then HSPICE automatically sets the plot limits. These limits
apply to the actual x-axis variable value, regardless of the
XSCAL type.
Default 0.0
XSCAL
Scale for the x-axis. Two common axis scales are: Linear(LIN)
(XSCAL=1)
Logarithm(LOG) (XSCAL=2) Default 1.0
YMIN, YMAX
■
If YMIN is not equal to YMAX, then YMIN and YMAX determine
the y-axis plot limits. The y-axis limits in the .GRAPH command
overrides YMIN and YMAX in the model.
■
If you do not specify plot limits, HSPICE sets the plot limits.
These limits apply to the actual y-axis variable value,
regardless of the YSCAL type.
Default 0.0
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
773
Appendix A: Obsolete Commands and Options
.MODEL Command for .GRAPH
774
Argument
Description
YSCAL
Scale for the y-axis. Two common axis scales are: Linear(LIN)
(XSCAL=1)
Logarithm(LOG) (XSCAL=2) Default 1.0
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.NET
.NET
OBSOLETE. Computes parameters for impedance, admittance, hybrid, and
scattering matrixes. This functionality is replaced by the .LIN command.
Syntax
One-Port Network
.NET input [RIN=val]
.NET input val
Two-Port Network
.NET output input [ROUT=val] [RIN=val]
Argument
Description
input
Name of the voltage or current source for AC input.
output
Output port. It can be:
■
■
An output voltage, V(n1[,n2]).
An output current, I (source), or I (element).
RIN
Input or source resistance. RIN calculates output impedance, output
admittance, and scattering parameters. The default RIN value is 1 ohm.
ROUT
Output or load resistance. ROUT calculates input impedance,
admittance, and scattering parameters. The default is 1 ohm.
Description
You can the .NET command to compute parameters for:
■
Z impedance matrix
■
Y admittance matrix
■
H hybrid matrix
■
S scattering matrix
You can use the .NET command only in conjunction with the .AC command.
HSPICE also computes:
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
775
Appendix A: Obsolete Commands and Options
.NET
■
Input impedance
■
Output impedance
■
Admittance
This analysis is part of AC small-signal analysis. To run network analysis,
specify the frequency sweep for the .AC command.
Examples
One-Port Network
.NET
.NET
VINAC
RIN=50
IIN
RIN=50
Two-Port Network
.NET V(10,30)
VINAC
ROUT=75
RIN=50
.NET I(RX)
VINAC
ROUT=75
RIN=50
776
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.PLOT
.PLOT
OBSOLETE. Plots the output values of one or more variables in a selected
HSPICE analysis as a low-resolution (ASCII) plot in the output listing file. This
is an obsolete command. You get the same functionality using the .PRINT
command.
Syntax
.PLOT antype ov1 [(plo1,phi1)] [ov2] [(plo2,phi2)] ...]
Argument
Description
antype
Type of analysis for the specified plots. Analysis types are: DC, AC,
TRAN, NOISE, or DISTO.
ov1 ...
Output variables to plot: voltage, current, or element template variables
(HSPICE only; HSPICE RF does not support element template output
or .PLOT commands) from a DC, AC, TRAN, NOISE, or DISTO
analysis. See the next sections for syntax.
plo1, phi1 ...
Lower and upper plot limits. The plot for each output variable uses the
first set of plot limits after the output variable name. Set a new plot limit
for each output variable after the first plot limit. For example to plot all
output variables that use the same scale, specify one set of plot limits
at the end of the .PLOT command. If you set the plot limits to (0,0)
HSPICE automatically sets the plot limits.
Description
Use this command to plot the output values of one or more variables in a
selected HSPICE analysis. Each .PLOT command defines the contents of one
plot, which can contain more than one output variable.
If more than one output variable appears on the same plot, HSPICE prints and
plots the first variable specified. To print out more than one variable, include
another .PLOT command. You can include wildcards in .PLOT commands.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
777
Appendix A: Obsolete Commands and Options
.PLOT
Examples
In Example 1,
■
In the first line, PAR plots the ratio of the collector current and the base
current for the Q1 transistor.
■
In the second line, the VDB output variable plots the AC analysis results (in
decibels) for node 5.
■
In the third line, the AC plot can include NOISE results and other variables
that you specify.
Example 1
.PLOT DC V(4) V(5) V(1) PAR(`I1(Q1)/I2(Q1)')
.PLOT TRAN V(17,5) (2,5) I(VIN) V(17) (1,9)
.PLOT AC VM(5) VM(31,24) VDB(5) VP(5) INOISE
In the last line of Example 2, HSPICE sets the plot limits for V(1) and V(2), but
you specify 0 and 5 volts as the plot limits for V(3) and V(4).
Example 2
.PLOT AC ZIN YOUT(P) S11(DB) S12(M) Z11(R)
.PLOT DISTO HD2 HD3(R) SIM2
.PLOT TRAN V(5,3) V(4) (0,5) V(7) (0,10)
.PLOT DC V(1) V(2) (0,0) V(3) V(4) (0,5)
778
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.WIDTH
.WIDTH
OBSOLETE. Specifies the width of the low resolution (ASCII) plot in the listing
file.
Syntax
.WIDTH OUT={80 |132}
Argument
Description
OUT
Output print width.
Description
Use this command to specify the width of the low resolution (ASCII) plot.
Permissible values for OUT are 80 and 132. You can also use .OPTION CO to
set the OUT value.
Examples
.WIDTH OUT=132 $ SPICE compatible style
.OPTION CO=132 $ preferred style
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
779
Appendix A: Obsolete Commands and Options
.OPTION ACCT
.OPTION ACCT
OBSOLETE. Generates a detailed accounting report.
Syntax
.OPTION ACCT
.OPTION ACCT=[1|2]
Default Default 1
Argument
Description
.OPTION ACCT
Enables reporting.
.OPTION ACCT=1 (default)
Is the same as ACCT without arguments.
.OPTION ACCT=2
Enables reporting and matrix statistic reporting.
Description
Obsolete with 2009.03 release (MT starts will be printed by default.) Use this
option to generate a detailed accounting report.
Examples
.OPTION ACCT=2
The ratio of TOT.ITER to CONV.ITER is the best measure of simulator
efficiency. The theoretical ratio is 2:1. In this example the ratio is 2.57:1. SPICE
generally has a ratio from 3:1 to 7:1.
In transient analysis, the ratio of CONV.ITER to # POINTS is the measure of
the number of points evaluated to the number of points printed. If this ratio is
greater than about 4:1, the convergence and time step control tolerances might
be too tight for the simulation.
780
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION ALT999 or ALT9999
.OPTION ALT999 or ALT9999
Allows the.GRAPH command to create more output files when you run .ALTER
simulations.
Syntax
.OPTION ALT999
.OPTION ALT9999
Description
Use this option to allow the.GRAPH command to create more output files when
you run .ALTER simulations.
This option is now obsolete. HSPICE can now generate up to 10,000 unique
files without using this option.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
781
Appendix A: Obsolete Commands and Options
.OPTION BKPSIZ
.OPTION BKPSIZ
OBSOLETE. Sets the size of the breakpoint table.
Syntax
.OPTION BKPSIZ=x
Default Default 5000
Description
Use this option to set the size of the breakpoint table. This is an obsolete
option, provided only for backward-compatibility.
782
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION CDS
.OPTION CDS
OBSOLETE. Produces a Cadence WSF (ASCII format) post-analysis file for
Opus♠ .
Syntax
.OPTION CDS=x
Description
Use this option to produce a Cadence WSF (ASCII format) post-analysis file for
Opus♠ when CDS=2. This option requires a specific license. The CDS option
is the same as the SDA option.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
783
Appendix A: Obsolete Commands and Options
.OPTION CO
.OPTION CO
OBSOLETE. Sets column width for printouts.
Syntax
.OPTION CO=column_width
Argument
Description
column_width
The number of characters in a single line of output.
Description
(Obsolete) Use this option to set the column width for printouts. The number of
output variables that print on a single line of output is a function of the number
of columns.
You can set up to 5 output variables per 80-column output, and up to 8 output
variables per 132-column output with 12 characters per column. HSPICE
automatically creates additional print commands and tables for all output
variables beyond the number that the CO option specifies. The default is 78.
Examples
* Narrow print-out (default)
.OPTION CO=80
* Wide print-out
.OPTION CO=132
784
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.DEGINFO
.DEGINFO
OBSOLETE with the D-2010.03 release. Generates the degradation
information during the transient simulation for user-specified MOSFET element
when used with the MOSRA API.
Syntax
.DEGINFO [YES|NO] MOSFET_instance_name1
+ MOSFET_instance_name2...
Default
YES
Argument
Description
YES|NO
YES: the MOSFETs in the instance name list will be recorded.
NO: the MOSFETs in the instance name list will NOT be recorded.
Description
Use this command to generate the degradation information during the transient
simulation for user-specified MOSFET element. A separate output file,
*.deginfo, is generated.
Examples
The command in Example 1 records the information of MN1 and MP2 in
the .deginfo file.
Example 1
.DEGINFO YES MN1 MP2
The command in Example 2 records the information of all of the MOSFETs
except MN3 and MP5.
Example 2
DEGINFO NO MN3 MP5
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
785
Appendix A: Obsolete Commands and Options
.OPTION H9007
.OPTION H9007
OBSOLETE. Sets default values for general-control options to correspond to
values for HSPICE H9007D.
Syntax
.OPTION H9007
Default
0
Description
Use this option to set default values for general-control options to correspond to
values for HSPICE H9007D. If you set this option, HSPICE does not use the
EXPLI model parameter.
786
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION MEASSORT
.OPTION MEASSORT
OBSOLETE. Automatically sorts large numbers of .MEASURE commands.
(This option is obsolete.)
Syntax
.OPTION MEASSORT=x
Default
0
Description
Starting in version 2003.09, this option is obsolete. Measure performance is
now order-independent and HSPICE ignores this option.
In versions of HSPICE before 2003.09, to automatically sort large numbers
of .MEASURE commands, you could use the .OPTION MEASSORT command.
■
.OPTION MEASSORT=0 (default; did not sort .MEASURE commands).
■
.OPTION MEASSORT=1 (internally sorted .MEASURE commands).
You needed to set this option to 1 only if you used a large number of .MEASURE
commands, where you needed to list similar variables together (to reduce
simulation time). For a small number of .MEASURE commands, turning on
internal sorting sometimes slowed-down simulation while sorting, compared to
not sorting first.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
787
Appendix A: Obsolete Commands and Options
.OPTION MENTOR
.OPTION MENTOR
OBSOLETE. Enables the Mentor MSPICE-compatible (ASCII) interface.
Syntax
.OPTION MENTOR=0|1|2
Default Default 0
Description
Use this option to enable the Mentor MSPICE-compatible (ASCII) interface.
MENTOR=2 enables that interface. This option requires a specific license.
788
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION MODSRH
.OPTION MODSRH
OBSOLETE. Made obsolete beginning in the 2008.03 release as it increases
runtime and costs more memory. Controls whether HSPICE loads or
references a model described in a .MODEL command, but not used in the
netlist.
Syntax
.OPTION MODSRH=0|1
Description
Use this option to control whether HSPICE loads or references a model
described in a .MODEL command, but is not used in the netlist.
This option parameter determines if HSPICE reads and loads every model card
or all model bins that are present in netlists and model libraries during a
simulation run. When this parameter is set to 0, all the model cards in the
model libraries are read into HSPICE even if there are certain models or bins
that are not referenced by any elements of the netlists. If this option parameter
is not assigned a numerical value or is set to 1, or it is not specified at all, then
only those model cards or model bins that are referenced are read into the
HSPICE executable for simulation.
Note:
The.OPTION MODSRH control must appear before the .MODEL
definition.
■
MODSRH=0: all models expanded even if the model described in a .MODEL
command is not referenced. This was the default prior to Y-2006.03 and
restored in A-2008.03.
■
MODSRH=1: only referenced models are expanded. This option shortens
simulation runtime when the netlist references many models, but no element
in the netlist calls those models. This option increased read-in time. This
became the default after 2008.03.
Examples
In this example, the input file automatically searches t6.inc for the nch model,
but it is not loaded.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
789
Appendix A: Obsolete Commands and Options
.OPTION MODSRH
example.sp:
.option post modsrh=1
xi1 net8 b c t6
xi0 a b net8 t6
v1 a 0 pulse 3.3 0.0 10E-6 1E-9 1E-9
+ 25E-6 50E-6
v2 b 0 2
v3 c 0 3
.model nch nmos level=49 version=3.2
.end
See Also
.MODEL
790
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION PIVREF
.OPTION PIVREF
OBSOLETE. Made obsolete with 2009.03 release. Sets a pivot reference.
Syntax
.OPTION PIVREF=x
Description
Use this option to set a pivot reference. Use PIVREF in PIVOT=11, 12, or 13 to
limit the size of the matrix. The default is 1e+8.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
791
Appendix A: Obsolete Commands and Options
.OPTION NOPAGE
.OPTION NOPAGE
OBSOLETE Suppresses page ejects for title headings.
Syntax
.OPTION NOPAGE=[0|1]
Description
Use this option to suppress page ejects for title headings.
792
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION PIVREL
.OPTION PIVREL
OBSOLETE (2009.03) release.Sets maximum and minimum ratio of a row or
matrix.
Syntax
.OPTION PIVREL=x
Description
Use this option to set the maximum and minimum ratio of a row or matrix. Use
only if PIVOT=1. Large values for PIVREL can result in very long matrix pivot
times; however, if the value is too small, no pivoting occurs. Start with small
values of PIVREL by using an adequate but not excessive value for
convergence and accuracy. The default is 1e-4.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
793
Appendix A: Obsolete Commands and Options
.OPTION PLIM
.OPTION PLIM
OBSOLETE. Made obsolete with 2009.03 release.Specifies plot size limits for
current and voltage plots.
Syntax
.OPTION PLIM
Default Default 0
Description
Use this option to specify plot size limits for current and voltage plots:
■
Finds a common plot limit and plots all variables on one graph at the same
scale.
■
Enables SPICE-type plots, which create a separate scale and axis for each
plot variable.
This option does not affect postprocessing of graph data.
794
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION SDA
.OPTION SDA
OBSOLETE. Produces a Cadence WSF (ASCII format) post-analysis file for
Opus♠ .
Syntax
.OPTION SDA=x
Default Default 0
Description
Use this option to produce a Cadence WSF (ASCII format) post-analysis file for
Opus♠ . Set SDA=2 to produce this file. This option requires a specific license.
The SDA is the same as the CDS option.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
795
Appendix A: Obsolete Commands and Options
.OPTION SPICE
.OPTION SPICE
Makes HSPICE compatible with Berkeley SPICE.
Syntax
.OPTION SPICE
Description
When the option SPICE is set, the following options and model parameters are
used:
General parameters used with .OPTION SPICE:
TNOM=27 DEFNRD=1 DEFNRS=1 INGOLD=2 ACOUT=0 DC
PIVOT PIVTOL=IE-13 PIVREL=1E-3 RELTOL=1E-3 ITL1=100
ABSMOS=1E-6 RELMOS=1E-3 ABSTOL=1E-12 VNTOL=1E-6
ABSVDC=1E-6 RELVDC=1E-3 RELI=1E-3
Transient parameters used with .OPTION SPICE:
DCAP=1 RELQ=1E-3 CHGTOL-1E-14 ITL3=4 ITL4=10 ITL5=5000
FS=0.125 FT=0.125
Model parameters used with .OPTION SPICE:
For BJT: MJS=0
For MOSFET, CAPOP=0
LD=0 if not user-specified
UTRA=0 not used by SPICE for level=2
NSUB must be specified
NLEV=0 for SPICE noise equation
796
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix A: Obsolete Commands and Options
.OPTION SIM_LA_MINMODE
.OPTION SIM_LA_MINMODE
Obsolete as of 2009.03. Reduces the number of nodes instead of the number
of elements.
Syntax
.OPTION SIM_LA_MINMODE=ON | OFF
Default Default OFF
Description
Use this option to reduce the number of nodes instead of the number of
elements.
■
ON: reduces the number of nodes
■
OFF: does not reduce the number of nodes.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
797
Appendix A: Obsolete Commands and Options
.OPTION ZUKEN
.OPTION ZUKEN
OBSOLETE. Enables or disables the Zuken interface.
Syntax
.OPTION ZUKEN=x
Description
Use this option to enable or disable the Zuken interface.
798
■
If x is 2, the interface is enabled.
■
If x is 1 (default), the interface is disabled.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
B
B
How Options Affect other Options
Describes the effects of specifying control options on other options in the netlist.
The following options either impact or are impacted by the specifying of other
.OPTION parameters:
■
GEAR Method
■
ACCURATE
■
FAST
■
GEAR Method, ACCURATE
■
ACCURATE, GEAR Method
■
ACCURATE, FAST
■
GEAR Method, FAST
■
GEAR Method, ACCURATE, FAST
■
RUNLVL=N
■
RUNLVL, ACCURATE, FAST, GEAR method
■
DVDT=1,2,3
■
LVLTIM=0,2,3
■
KCLTEST
■
BRIEF
■
Option Notes
■
Finding the Golden Reference for Options
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
799
Appendix B: How Options Affect other Options
GEAR Method
GEAR Method
Specifying .OPTION METHOD=GEAR sets the values of other options as
follows:
■
BYPASS = 0
■
BYTOL = 50u
■
DVDT = 3
■
LVLTIM = 2
■
MBYPASS = 1.0
■
METHOD = 2
■
RMAX = 2.0
■
SLOPETOL = 500m
ACCURATE
Specifying the ACCURATE option sets the values of other options as follows:
■
ABSVAR = 0.2
■
ACCURATE =1
■
BYPASS = 2
■
DVDT = 2
■
FFT_ACCU = 1
■
FT = 0.2
■
LVLTIM = 3
■
RELMOS = 0.01
■
RELVAR = 0.2
FAST
Specifying the FAST option sets the values of other options as follows:
800
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix B: How Options Affect other Options
GEAR Method, ACCURATE
■
BYTOL = 50u
■
DVDT = 3
■
BYPASS = 0
■
DVDT = 2
■
FAST = 1
■
MBYPASS = 1.0
■
RMAX = 2.0
■
SLOPETOL = 500m
GEAR Method, ACCURATE
Specifying .OPTION METHOD=GEAR first with the ACCURATE option sets
the values of other options as follows:
■
ABSVAR = 0.2
■
ACCURATE =1
■
BYPASS = 2
■
BYTOL = 50u
■
DVDT = 2
■
FFT_ACCU = 1
■
FT = 0.2
■
LVLTIM = 3
■
MBYPASS = 1.0
■
METHOD = 2
■
RELMOS = 0.01
■
RELVAR = 0.2
■
RMAX = 2
■
SLOPETOL = 500m
Note:
When GEAR is specified first, DVDT=2 and LVLTIM=3.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
801
Appendix B: How Options Affect other Options
ACCURATE, GEAR Method
ACCURATE, GEAR Method
Specifying the ACCURATE option first in with .OPTION METHOD=GEAR sets
the values of other options as follows:
■
ABSVAR = 0.2
■
ACCURATE =1
■
BYPASS = 2
■
BYTOL = 50u
■
DVDT = 3
■
FFT_ACCU = 1
■
FT = 0.2
■
LVLTIM = 2
■
MBYPASS = 1.0
■
METHOD = 2
■
RELMOS = 0.01
■
RELVAR = 0.2
■
RMAX = 2
■
SLOPETOL = 500m
Note:
When ACCURATE is specified before the GEAR method, then
DVDT=2, LVLTIM=3.
ACCURATE, FAST
Specifying the ACCURATE option with the FAST option sets the values of other
options as follows:
802
■
ABSVAR = 0.2
■
ACCURATE =1
■
BYPASS = 2
■
BYTOL = 50u
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix B: How Options Affect other Options
GEAR Method, FAST
■
DVDT = 2
■
FAST = 1
■
FFT_ACCU = 1
■
FT = 0.2
■
LVLTIM = 3
■
MBYPASS = 1.0
■
RELMOS = 0.01
■
RELVAR = 0.2
■
RMAX = 2
■
SLOPETOL = 500m
Note:
The ACCURATE and FAST options are order-independent.
GEAR Method, FAST
Specifying .OPTION METHOD=GEAR in combination with the FAST option
sets the values of other options as follows:
■
BYTOL = 50u
■
DVDT = 3
■
FAST = 1
■
LVLTIM = 2
■
MBYPASS = 2
■
METHOD = 0.01
■
RMAX = 2
■
SLOPETOL = 500m
Note:
The METHOD=GEAR and FAST options are order-independent.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
803
Appendix B: How Options Affect other Options
GEAR Method, ACCURATE, FAST
GEAR Method, ACCURATE, FAST
Specifying .OPTION METHOD=GEAR first in combination with the ACCURATE
and FAST options sets the values of other options as follows:
■
ABSVAR = 0.2
■
ACCURATE =1
■
BYPASS = 2
■
BYTOL = 50u
■
DVDT = 2
■
FAST = 1
■
FFT_ACCU = 1
■
FT = 0.2
■
LVLTIM = 3
■
METHOD = 2
■
MBYPASS = 1.0
■
RELMOS = 0.01
■
RELVAR = 0.2
■
RMAX = 2
■
SLOPETOL = 500m
Note:
If GEAR is specified first, then DVDT=2 LVLTIM=3. Otherwise,
the METHOD=GEAR, ACCURATE, and FAST options are orderindependent.
RUNLVL=N
Specifying the RUNLVL option with any legal numeric value sets the following
options:
804
■
BYPASS = 2 (If METHOD=GEAR with RUNLVL=0, then BYPASS=0)
■
DVDT = 3
■
LVLTIM = 4
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix B: How Options Affect other Options
RUNLVL, ACCURATE, FAST, GEAR method
■
RUNLVL = N
■
SLOPETOL = 500m
RUNLVL, ACCURATE, FAST, GEAR method
Specifying the options RUNLVL, ACCURATE, and FAST with METHOD=GEAR
is order-independent:
■
RUNLVL option (LVLTIM = 4) is always on
■
GEAR method is always selected
■
RUNLVL = 5 is always selected
■
FAST has no effect on RUNLVL
DVDT=1,2,3
Specifying the DVDT option= 1,2,3 sets the following options:
■
BYPASS = 0
■
BYTOL = 50u
■
MBYPASS = 1.0
■
RMAX = 2
■
SLOPETOL = 500m
LVLTIM=0,2,3
Specifying the LVLTIM option= 1,2,3 sets the following options:
■
BYPASS = 0
■
BYTOL = 50u
■
MBYPASS = 1.0
■
RMAX = 2
■
SLOPETOL = 500m
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
805
Appendix B: How Options Affect other Options
KCLTEST
These options are order-independent.
Note:
The DVDT value is ignored if LVLTIM = 2
KCLTEST
Specifying the KCLTEST option sets the following options:
■
ABSTOL = 1u
■
RELI = 1u
KCLTEST is order-dependent with ABSTOL and RELI.
BRIEF
Specifying the BRIEF option resets the following options to their defaults:
■
NODE
■
LIST
■
OPTS
and sets the NOMOD option.
The BRIEF option is order-dependent with the affected options. If option BRIEF
is specified after NODE, LIST, OPTS, and NOMOD, then it resets them. If
option BRIEF is specified before NODE, LIST, OPTS, and NOMOD, then those
options overwrite whatever values option BRIEF may have set.
Option Notes
806
■
ABSTOL aliases ABSI
■
VNTOL aliases ABSV
■
If ABSVDC is not set, VNTOL sets it
■
DCTRAN aliases CONVERGE
■
GMIN does not overwrite GMINDC, nor does GMINDC overwrite GMIN
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Appendix B: How Options Affect other Options
Option Notes
■
RELH only takes effect when ABSH is non-zero
■
RELTOL aliases RELV
■
RELVDC defaults to RELTOL
■
If RELTOL < BYTOL, BYTOL = RELTOL
■
RELVAR applies to LVLTIM = 1 or 3 only
■
CHGTOL, RELQ & TRTOL are the only error tolerance options for
LVLTIM = 2 (LTE)
■
The DVDT algorithm works with LVLTIM = 1 and 3
RUNLVL Option Notes
If RUNLVL is invoked, you can disable it by:
■
Adding .OPTION RUNLVL=0 to your current simulation job.
■
Copying $installdir/hspice.ini to your HOME directory and customize it by
adding .OPTION RUNLVL=0, which disables it for all of your simulation jobs.
■
Re-invoking the $installdir/bin/config program and deselecting the option
runlvl setting in box 'hspice.ini' which disables it for the whole group of
simulation jobs.
If RUNLVL is invoked, some options are ignored or automatically set:
Options below are automatically set (user setting will overwrite them):
■
If runlvl=6, then .option bypass=0
■
If runlvl=1|2|3|4|5, then .option bypass=2
■
The following options are ignored; they are replaced by automated
algorithms: lvltim, dvdt, ft, fast, trtol, absvar, relvar, relq, chgtol, dvtr, imin,
itl3, rmax
If RUNLVL is invoked, actual values of options used by HSPICE are:
■
runlvl= 3
■
bypass= 2
■
mbypass= 2.00
■
bytol= 100.00u
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
807
Appendix B: How Options Affect other Options
Finding the Golden Reference for Options
■
bdfatol=1e-3
■
bdfrtol=1e-3
Finding the Golden Reference for Options
When trying to determine the acceptable trade-off between HSPICE accuracy
and transient analysis simulation performance, it is important to first establish a
reference value for the measurements you are using to evaluate the
performance (speed and accuracy) of a given HSPICE configuration. There are
multiple ways to configure HSPICE for higher accuracy. The following is a good
starting point that you might want to modify for your specific application:
.OPTION RUNLVL=6 ACCURATE KCLTEST DELMAX=a_small_value
The options are described as follows:
808
Options
Description
RUNLVL
Invokes the RUNLVL algorithm and sets tolerances to their tightest
values. Refer to .OPTION RUNLVL for more details:
ACCURATE
Sets even more HSPICE OPTIONs to tighter tolerances.
(See .OPTION ACCURATE for details.
KCLTEST
Activates Kirchhoff's Current Law testing for every circuit node.
(See .OPTION KCLTEST for details.
DELMAX
Sets the largest timestep that HSPICE is allowed to take. It should
be set to the smallest value (1ps, for example) that still allows the
simulation to finish in a reasonable amount of time. Typically, it
should be set approximately
1/(20*highest-frequency-activity-in-the-circuit)
Warning: This option can create very large tr0 files. Be careful to
only probe the needed nodes (use .OPTION PROBE combined with
.PROBE). See .OPTION DELMAX for details.
HSPICE® Reference Manual: Commands and Control Options
E-2010.12
Index
Symbols
(X0R, X0I) option 727
(X1R, X1I) option 728
(X2R, X2I) option 729
A
ABSH option 352
ABSI option 353, 514
ABSMOS option 355, 514
ABSOUT optimization bisection parameter 216
ABSTOL option 356
ABSV option 357
ABSVAR option 358
ABSVDC option 359
AC analysis
magnitude 361
optimization 25
output 361
phase 361
.AC command 25
external data 65
ACCT option 780
ACCURATE option 360
combined with FAST option 802
combined with FAST option and GEAR method
804
combined with GEAR option 801, 802
plus FAST and RUNLVL options and
METHOD=GEAR 805
.ACMATCH command 28
ACOUT option 361
algorithms
DVDT 358, 531
local truncation error 531, 616, 708
pivoting 594
timestep control 448
transient analysis timestep 531
trapezoidal integration 546
.ALIAS command 31
ALL keyword 233, 266
ALT9999 option 781
ALTCC option 362
ALTCHK option 363
alter block commands 15
ALTER cases, multiprocessing 5
.ALTER command 33, 81
Analog Artist interface 603
See also Artist
Analysis commands 14
analysis, network 776
APPENDALL option 364
.APPENDMODEL 35
arguments, command-line
hspice 2
hspicerf 12
arithmetic expression 185
ARTIST option 366
ASCII output 12
ASCII output data 544, 783, 795
ASPEC option 367
AT keyword 175, 180
AUTOSTOP option 368
average nodal voltage, with .MEASURE 187
average value, measuring 188
AVG keyword 187, 199
B
BADCHR option 387, 392
BETA keyword 265
.BIASCHK command 38
BIASFILE option 393
BIASINTERVAL option 394
BIASNODE option 395
BIASPARALLEL option 396
BIAWARN option 397
BINPRNT option 398
bisection
pushout 203
BKPSIZ option 782
809
Index
C
BPNMATCHTOL option 399
branch current error 353
breakpoint table, size 782
BRIEF option 233, 236, 400, 526, 565, 574, 581
effect on other options 806
BSIM4PDS option 401
bus notation 759
BYPASS option 402
BYTOL option 403
C
Cadence
Opus 783, 795
WSF format 783, 795
capacitance
charge tolerance, setting 406
CSHUNT node-to-ground 417
table of values 404
capacitor, models 214
CAPTAB option 404
CDS option 783
.CFL_PROTOTYPE 44
C-function library 44
characterization of models 73
charge tolerance, setting 406
.CHECK EDGE command 48
.CHECK FALL command 50
.CHECK GLOBAL_LEVEL command 51
.CHECK HOLD command 52
.CHECK IRDROP command 54
.CHECK RISE command 56
.CHECK SETUP command 58
.CHECK SLEW command 59
CHGTOL option 406
CLOSE optimization parameter 215
CMIFLAG option 408
CMIPATH option 409
CMIUSRFLAG option 410
CO option 314, 317, 779, 784
column laminated data 69
command-line arguments
hspice 2
hspicerf 12
commands
.AC 25
.ACMATCH 28
810
.ALIAS 31
.ALTER 33, 81
alter block 15
analysis 14
.APPENDMODEL 35
.BIASCHK 38
.CFL_PROTOTYPE 44
.CHECK EDGE 48
.CHECK FALL 50
.CHECK GLOBAL_LEVEL 51
.CHECK HOLD 52
.CHECK IRDROP 54
.CHECK RISE 56
.CHECK SETUP 58
.CHECK SLEW 59
.CONNECT 61
.DATA 64
.DC 71
.DCMATCH 76
.DCVOLT 80
.DEL LIB 81
.DISTO 86
.DOUT 88
.EBD 90
.ELSE 92
.ELSEIF 93
.END 94
.ENDDATA 95
.ENDIF 96
.ENDL 97
.ENDS 98
.ENV 99
.ENVFFT 100
.ENVOSC 101
.EOM 102
.FFT 103
.FLAT 108
.FOUR 110
.FSOPTIONS 111
.GLOBAL 114
.GRAPH 771
.HB 115
.HBAC 118
.HBLIN 119
.HBLSP 121
.HBNOISE 123
.HBOSC 126
.HBXF 131
Index
C
.HDL 132
.IBIS 134
.IC 138
.ICM 140
.IF 142
.INCLUDE 144
.LAYERSTACK 148
.LIB 150
.LIN 154
.LOAD 158
.LPRINT 160
.MACRO 164
.MALIAS 167
.MATERIAL 169
.MEASURE 171
.MEASURE PHASENOISE 198, 199
.MEASURE PTDNOISE 202
.MEASURE(ACMATCH) 205
.MEASURE(DCMATCH) 206
.MODEL 213
.MOSRA 222
.MOSRAPRINT 226
.NET 775
.NODESET 228
.NOISE 230
.OP 233
.OPTION 235
.PARAM 237
.PAT 241
.PHASENOISE 244
.PKG 247
.PLOT 777
.POWER 249
.POWERDC 251
.PRINT 252
.PROBE 255
.PROTECT 258
.PTDNOISE 259
.PZ 263
.SAVE 266
.SENS 268
.SHAPE 270
.SNFT 280
.SNOSC 285
.SNXF 288
.STATEYE 290
.STIM 294
subcircuit 18
.SUBCKT 301
.SURGE 306
.SWEEPBLOCK 307
.TEMP (or) .TEMPERATURE 309
.TF 312
.TITLE 313
.TRAN 314
.UNPROTECT 324
.VARIATION 325
.VEC 327
Verilog-A 19
.WIDTH 779
Common Simulation Data Format 446
concatenated data files 68
Conditional Block 15
conductance
current source, initialization 465
minimum, setting 466
models 427
MOSFETs 467
negative, logging 445
node-to-ground 471
sweeping 468
.CONNECT command 61
control options
printing 581
setting 236
transient analysis
limit 712
CONVERGE option 412, 428
convergence
for optimization 216
problems
changing integration algorithm 546
CONVERGE option 412, 428
DCON setting 426
decreasing the timestep 459
operating point Debug mode 233
steady state 468
CPTIME option 413
CPU time, reducing 566
CROSS keyword 179, 183
CSCAL option 414, 529
CSDF option 415
CSHDC option 416
CSHUNT option 417
current
ABSMOS floor value for convergence 615
811
Index
D
branch 353
operating point table 233
CURRENT keyword 233
current threshold option 513
CUSTCMI option 418
CUT optimization parameter 216
CVTOL option 419
D
-d argument 3
D_IBIS option 420
.DATA command 64
datanames 66
external file 64
for sweep data 65
inline data 66
data files, disabling printout 400, 574
DATA keyword 25, 65, 71, 315
datanames 66, 295
DC
analysis
decade variation 72
initialization 424
iteration limit 505
linear variation 72
list of points 72
octave variation 72
optimization 71
.DC command 71, 73
external data with .DATA 65
DCAP option 421
DCCAP option 422
DCFOR option 423
DCHOLD option 424
DCIC option 425
.DCMATCH command 76
DCON option 426
DCSTEP option 427
DCTRAN option 428
.DCVOLT command 80, 138
DEBUG keyword 233
DEC keyword 26, 72, 316
DEFAD option 429
DEFAS option 430
DEFL option 431
DEFNRD option 432
812
DEFNRS option 433
DEFPD option 434
DEFPS option 435
DEFSA option 436
DEFSB option 437
DEFSD option 438
DEFW option 439
.DEL LIB command 81
with .ALTER 81
with .LIB 81
delays
group 709
DELMAX option 443, 627
DELTA internal timestep
See also timestep
demo files
MOSFETs 27
transmission (W-element) lines 113, 149, 170,
270
derivative function 193
DERIVATIVE keyword 193
derivatives, measuring 180
DI option 444
DIAGNOSTIC option 445
DIFSIZ optimization parameters 216
digits, significant 539
diode models 214
.DISTO command 86
distributed processing 5
DLENCSDF option 446
.DOUT command 88
DP option 5
DV option 426, 447
DVDT
algorithm 358
option 448, 531
DVDT option 448
DVDToption
value e1,2,3 ffect on other options
.OPTION DVDT
value 1,2,3 effect on other options
805
DVTR option 449
E
.EBD command 90
Index
F
element
checking, suppression of 566
OFF parameter 575
.ELSE command 92
.ELSEIF command 93
EM_RECOVERY option 451
ENABLE command 736
Encryption 16
.END command 94
for multiple HSPICE runs 94
location 94
.ENDDATA command 95
ENDDATA keyword 64, 68
.ENDIF command 96
.ENDL command 97, 151
.ENDS command 98
.ENV command 99
envelope simulation 99
FFT on output 100
oscillator startup, shutdown 101
.ENVFFT command 100
.ENVOSC command 101
.EOM command 102
EPSMIN option 452
equation 185
ERR function 196, 197
ERR1 function 196
ERR2 function 196
ERR3 function 196
error function 196
errors
branch current 353
function 197
internal timestep too small 417, 628
optimization goal 174
tolerances
ABSMOS 355
branch current 353
RELMOS 355
EXPLI option 453
EXPMAX option 454
expression, arithmetic 185
external data files 66
F
FALL keyword 179, 183
fall time
verification 50
FAST option 455
effect on other options 800
FASToption
combined with ACCURATE option 802
combined with ACCURATE option and GEAR
method 804
combined with GEAR method 803
plus ACCURATE and RUNLVL options and
METHOD=GEAR 805
.FFT command 103
FFT_ACCURATE option 456
FFTOUT option 457
FIL keyword 66
files
column lamination 69
concatenated data files 68
filenames 66
hspice.ini 544
include files 144, 152
input 2
multiple simulation runs 94
output
version number 3, 12
FIND keyword 180
FIND, using with .MEASURE 178
.FLAT command 108
floating point overflow
CONVERGE setting 412
setting GMINDC 467
FMAX option 458
.FOUR command 110
FREQ
model parameter 773
frequency
ratio 86
sweep 27
FROM parameter 196
FS option 265, 459
FSCAL option 460
.FSOPTIONS command 111
FT option 461
functions
ERR 197
ERR1 196
ERR2 196
ERR3 196
813
Index
G
error 196
G
GDCPATH option 462
GEAR method
combined with FAST option 803
effect on options 800
GEAR option
combined with ACCURATE option 801, 802
effect on other options 800
GENK option 463
GEOSHRINK option 464
.GLOBAL command 114
global node names 114
GMAX option 465
GMIN option 466, 467
GMINDC option 467
GOAL keyword 188
GRAD optimization parameter 216
GRAMP
calculation 426
option 468
.GRAPH command 771
graph data file (Viewlogic format) 446
ground bounce checking 54
group delay, calculating 709
GSCAL option 469
GSHDC option 470
GSHUNT option 471
H
-h argument
usage information 12
H9007 option 786
harmonic balance analysis 116
harmonic balance noise analysis 125
harmonic balance transfer analysis 131, 288
harmonic balance-based periodic AC analysis 118
.HB command 115
HB_GIBBS option 478
.HBAC command 118
HBACKRYLOVDIM option 472
HBACKRYLOVITR option 473
HBACTOL option 474
HBCONTINUE option 475
814
HBFREQABSTOL option 476
HBFREQRELTOL option 477
HBJREUSE option 479
HBJREUSETOL option 480
HBKRYLOVDIM option 481
HBKRYLOVMAXITER option 483
HBKRYLOVTOL option 482
.HBLIN command 119
HBLINESEARCHFAC option 484
.HBLSP command 121
HBMAXITER option 485
.HBNOISE command 123
.HBOSC command 126
HBOSCMAXITER option 486
HBPROBETOL option 487
HBSOLVER option 488
HBTOL option 489
HBTRANFREQSEARCH option 490
HBTRANINIT option 491
HBTRANPTS option 492
HBTRANSTEP option 493
.HBXF command 131
HCI and NBTI analysis 225
.HDL command 132
HIER_DELIM option 494
HIER_SCALE option 495
HSPICE
job statistics report 780
version
H9007 compatibility 786
hspice
arguments 2
command 2
hspice.ini file 544
hspicerf
arguments 12
command 12
-html argument 3
I
-I argument 4
-i argument 2
.IBIS command 134
IBIS commands 17
.IC command 80, 138
Index
J
from .SAVE 267
IC keyword 266
IC parameter 80
.ICM command 140
ICSWEEP option 498
IDELAY command 737
.IF command 142
IGNOR keyword 196
IMAX option 499, 508
IMIN option 500, 507
.INCLUDE command 144
include files 144, 152
indepout 295
indepvar 295
inductors, mutual model 214
INGOLD option 501, 539
initial conditions
saving and reusing 498
initialization 575
inline data 66
input
data
adding library data 81
column laminated 69
concatenated data files 68
deleting library data 81
external, with .DATA command 65
filenames on networks 70
formats 66, 69
include files 144
printing 526
suppressing printout 526
file names 2
netlist file 94
INTEG keyword 187, 191, 199
used with .MEASURE 187
integral function 191
integration
backward Euler method 535
interfaces
Analog Artist 603
Mentor 788
MSPICE 788
ZUKEN 798
INTERP option 503
IO command 739
iterations
limit 505
maximum number of 509
ITL1 option 505
ITL2 option 506
ITL3 option 507
ITL4 option 508
ITL5 option 509
ITLPTRAN option 510
ITLPZ option 511
ITROPT optimization parameter 216
ITRPRT option 512
IVTH option 513
J
Jacobian data, printing 579
K
KCLTEST option 514
KCLTESToption
effect on other options
.OPTION KCLTEST
effect on other options 806
keywords
.AC command parameter 25
ALL 233, 266
AT 175, 180
AVG 187, 199
BETA 265
CROSS 179, 183
CURRENT 233
DATA 25, 65, 71, 315
.DATA command parameter 65
.DC command parameter 71
DEBUG 233
DEC 26, 72, 316
DERIVATIVE 193
ENDDATA 64, 68
FALL 179, 183
FIL 66
FIND 180
FS 265
IGNOR 196
INTEG 187, 191, 199
LAM 66, 69
LAST 179, 184
LIN 26, 72, 316
815
Index
L
MAXFLD 265
.MEASUREMENT command parameter 187,
199
MER 66, 69
MINVAL 196
MODEL 71
MONTE 26, 72, 315
NONE 233, 266
NUMF 265
OCT 26, 72, 316
OPTIMIZE 72
POI 26, 72, 316
PP 187, 199
RESULTS 72
RIN 775
RISE 179, 183
START 315
SWEEP 26, 72, 315
target syntax 175, 180
TO 188, 191, 197
TOL 265
TOP 266
.TRAN command parameter 315
TRIG 173
VOLTAGE 233
WEIGHT 188, 196
weight 188
WHEN 180
Kirchhoff’s Current Law (KCL) test 514
KLIM option 515
L
LA_FREQ option 516
LA_MAXR option 517
LA_MINC option 518
LA_TIME option 519
LA_TOL option 520
LAM keyword 66, 69
laminated data 69
LAST keyword 179, 184
latent devices
excluding 455
.LAYERSTACK command 148
LENNAM option 521
.LIB command 150
call command 150
in .ALTER blocks 151
816
nesting 151
with .DEL LIB 81
libraries
adding with .LIB 81
building 151
deleting 81
private 258
protecting 258
Library Management 17
LIMPTS option 522
LIMTIM option 523
.LIN command 154
LIN keyword 26, 72, 316
LIST option 526
listing, suppressing 258
.LOAD command 158
LOADHB option 527
LOADSNINIT option 528
local truncation error algorithm 531, 616, 708
.LPRINT command 160
LVLTIM option 531, 708
value 0,2,3 effect on other options 805
M
MACMOD option 532
.MACRO command 164
macros 81
magnetic core models 214
.MALIAS command 167
.MATERIAL command 169
Material Properties 16
matrix
minimum pivot values 595
parameters 775
row/matrix ratio 793
size limitation 791
MAX 187
MAX parameter 187, 199, 215
MAXAMP option 534
MAXFLD keyword 265
maximum value, measuring 188
MAXORD option 535
MBYPASS option 537
MCBRIEF option 538
MEASDGT option 539
Index
N
MEASFAIL option 540
MEASFILE option 541
MEASOUT option 544
MEASSORT option 787
.MEASURE command 171, 539, 544
average nodal voltage 187
expression 185
propogation delay 173
.MEASURE PHASENOISE 198, 199
.MEASURE(ACMATCH) command 205
.MEASURE(DCMATCH) command 206
measuring average values 188
measuring derivatives 180
Mentor interface 788
MENTOR option 788
MER keyword 66, 69
messages
See also errors, warnings
METHOD option 546
MIN 187
MIN parameter 187, 199
minimum value, measuring 188
MINVAL keyword 196
.MODEL command 213
ABSOUTT 216
CLOSE 215
CUT 216
DEV 217
DIFSIZ 216
distribution 217
GRAD 216
ITROPT 216
keyword 217
LOT 217
MAX 215
model name 213
PARMIN 216
RELIN 216
RELOUT 216
type 214
.MODEL command for .GRAPH 773
MODEL keyword 71
model parameters
.GRAPH command parameters 773
MONO 773
output 773
suppressing printout of 568
TEMP 309
TIC 773
models
BJTs 214
capacitors 214
characterization 73
diode 214
JFETs 214
magnetic core 214
MOSFETs 214
mutual inductors 214
names 213
npn BJT 214
op-amps 214
optimization 214
plot 214
private 258
protecting 258
simulator access 151
types 214
models, diode 214
MODMONTE option 549
MODSRH option 789
MONO model parameter 773
Monte Carlo
AC analysis 25
DC analysis 71
.MODEL parameters 217
time analysis 314
MONTE keyword 26, 72, 315
MONTECON option 553
.MOSRA command 222
MOSRALIFE option 554
.MOSRAPRINT command 226
MOSRASORT option 555
MSPICE simulator interface 788
-mt argument 5, 6
MTTHRESH option 560
MU option 561
multiprocessing, ALTER cases 5
multithreading, lowering device number threshold
560
N
-n argument 3, 12
namei 295
817
Index
O
NBTI and HCI analysis 225
NCFILTER option 562
n-channel, MOSFET’s models 214
NCWARN option 563
negative conductance, logging 445
nested library calls 151
.NET comamnd 775
network
analysis 776
filenames 70
network analysis 776
NEWTOL option 564
Node Naming 17
NODE option 565
nodes
cross-reference table 565
global versus local 114
printing 565
.NODESET command 228
from .SAVE 267
NODESET keyword 266
NOELCK option 566
noise
folding 265
numerical 417
sampling 265
.NOISE command 230
NOISEMINFREQ option 567
NOMOD option 568
NONE keyword 233, 266
NOPAGE option 792
NOPIV option 569
NOTOP option 570
NOWARN option 571
npn BJT models 214
npoints 295
NUMDGT option 572
numerical integration algorithms 546
numerical noise 417, 471
NUMERICAL_DERIVATIVES option 573
NUMF keyword 265
NXX option 574
O
OCT keyword 26, 72, 316
818
ODELAY command 740
OFF option 575
.OP command 233
op-amps model, names 214
operating point
capacitance 404
.IC command initialization 80
restoring 158
solution 575
voltage table 233
OPFILE option 576
OPTCON option 577
optimization
AC analysis 25
DC analysis 71
error function 174
iterations 216
models 214
time
analysis 315
optimization parameter, DIFSIZ 216
OPTIMIZE keyword 72
.OPTION (X0R, X0I) 727
.OPTION (X1R, X1I) 728
.OPTION (X2R, X2I) 729
.OPTION ABSH 352
.OPTION ABSI 353
.OPTION ABSMOS 355
.OPTION ABSTOL 356
.OPTION ABSV 357
.OPTION ABSVAR 358
.OPTION ABSVDC 359
.OPTION ACCT 780
.OPTION ACCURATE 360
combined with FAST option 802
combined with FAST option and GEAR method
804
combined with GEAR option 801, 802
plus FAST and RUNLVL options,
METHOD=GEAR 805
.OPTION ACOUT 361
.OPTION ALT9999 781
.OPTION ALTCC 362
.OPTION ALTCHK 363
.OPTION APPENDALL 364
.OPTION ARTIST 366
.OPTION ASPEC 367
Index
O
.OPTION AUTOSTOP 368
.OPTION BADCHR 387, 392
.OPTION BDFATOL 388, 390
.OPTION BIASFILE 393
.OPTION BIASINTERVAL 394
.OPTION BIASNODE 395
.OPTION BIASPARALLEL 396
.OPTION BIAWARN 397
.OPTION BINPRNT 398
.OPTION BISAAC 354
.OPTION BKPSIZ 782
.OPTION BPNMATCHTOL 399
.OPTION BRIEF 233, 236, 400, 526, 565, 574,
581
effect on other options 806
.OPTION BSIM4PDS 401
.OPTION BYPASS 402
.OPTION BYTOL 403
.OPTION CAPTAB 404
.OPTION CDS 783
.OPTION CHGTOL 406
.OPTION CMIFLAG 408
.OPTION CMIPATH 409
.OPTION CMIUSRFLAG 410
.OPTION CO 314, 317, 779, 784
.OPTION command 235
.OPTION CONVERGE 412
.OPTION CPTIME 413
.OPTION CSCAL 414, 529
.OPTION CSDF 415
.OPTION CSHDC 416
.OPTION CSHUNT 417
.OPTION CUSTCMI 418
.OPTION CVTOL 419
.OPTION D_IBIS 420
.OPTION DCAP 421
.OPTION DCCAP 422
.OPTION DCFOR 423
.OPTION DCHOLD 424
.OPTION DCIC 425
.OPTION DCSTEP 427
.OPTION DCTRAN 428
.OPTION DEFAD 429
.OPTION DEFAS 430
.OPTION DEFL 431
.OPTION DEFNRD 432
.OPTION DEFNRS 433
.OPTION DEFPD 434
.OPTION DEFPS 435
.OPTION DEFSA 436
.OPTION DEFSB 437
.OPTION DEFSD 438
.OPTION DEFW 439
.OPTION DELMAX 443
.OPTION DI 444
.OPTION DIAGNOSTIC 445
.OPTION DLENCSDF 446
.OPTION DV 447
.OPTION DVDT 448
.OPTION DVTR 449
.OPTION EM_RECOVERY 451
.OPTION EPSMIN 452
.OPTION EXPLI 453
.OPTION EXPMAX 454
.OPTION FAST 455
combined with ACCURATE option 802
combined with ACCURATE option and GEAR
method 804
combined with GEAR method 803
effect on other options 800
plus ACCURATE and RUNLVL options and
METHOD=GEAR 805
.OPTION FFT_ACCURATE 456
.OPTION FFTOUT 457
.OPTION FMAX 458
.OPTION FS 459
.OPTION FSCAL 460
.OPTION FT 461
.OPTION GDCPATH 462
.OPTION GEAR
combined with ACCURATE option 801, 802
effects on other options 800
.OPTION GENK 463
.OPTION GEOSHRINK 464
.OPTION GMAX 465
.OPTION GMIN 466
.OPTION GMINDC 467
.OPTION GRAMP 468
.OPTION GSCAL 469
.OPTION GSHDC 470
.OPTION GSHUNT 471
819
Index
O
.OPTION H9007 786
.OPTION HB_GIBBS 478
.OPTION HBACKRYLOVDIM 472
.OPTION HBACKRYLOVITR 473
.OPTION HBACTOL 474
.OPTION HBCONTINUE 475
.OPTION HBFREQABSTOL 476
.OPTION HBFREQRELTOL 477
.OPTION HBJREUSE 479
.OPTION HBJREUSETOL 480
.OPTION HBKRYLOVDIM 481
.OPTION HBKRYLOVMAXITER 483
.OPTION HBKRYLOVTOL 482
.OPTION HBLINESEARCHFAC 484
.OPTION HBMAXITER 485
.OPTION HBMAXOSCITER 486
.OPTION HBPROBETOL 487
.OPTION HBSOLVER 488
.OPTION HBTOL 489
.OPTION HBTRANFREQSEARCH 490
.OPTION HBTRANINIT 491
.OPTION HBTRANPTS 492
.OPTION HBTRANSTEP 493
.OPTION HIER_DELIM 494
.OPTION HIER_SCALE 495
.OPTION ICSWEEP 498
.OPTION IMAX 499
.OPTION IMIN 500
.OPTION INGOLD 501
.OPTION INTERP 503
.OPTION ITL1 505
.OPTION ITL2 506
.OPTION ITL3 507
.OPTION ITL4 508
.OPTION ITL5 509
.OPTION ITLPTRAN 510
.OPTION ITLPZ 511
.OPTION ITRPRT 512
.OPTION IVTH 513
.OPTION KCLTEST 514
.OPTION KLIM 515
.OPTION LA_FREQ 516
.OPTION LA_MAXR 517
.OPTION LA_MINC 518
.OPTION LA_TIME 519
820
.OPTION LA_TOL 520
.OPTION LENNAM 521
.OPTION LIMPTS 522
.OPTION LIMTIM 523
.OPTION LIST 526
.OPTION LOADHB 527
.OPTION LOADSNINIT 528
.OPTION LVLTIM 531
value 0,2,3 effect on other options 805
.OPTION MACMOD 532
.OPTION MAXAMP 534
.OPTION MAXORD 535
.OPTION MBYPASS 537
.OPTION MCBRIEF 538
.OPTION MEASDGT 539
.OPTION MEASFAIL 540
.OPTION MEASFILE 541
.OPTION MEASOUT 544
.OPTION MEASSORT 787
.OPTION MENTOR 788
.OPTION METHOD 546
.OPTION METHOD=GEAR
combined with FAST option 803
effects on other options 800
.OPTION MODMONTE 549
.OPTION MODSRH 789
.OPTION MONTECON 553
.OPTION MTTHRESH 560
.OPTION MU 561
.OPTION NCFILTER 562
.OPTION NCWARN 563
.OPTION NEWTOL 564
.OPTION NODE 565
.OPTION NOELCK 566
.OPTION NOISEMINFREQ 567
.OPTION NOMOD 568
.OPTION NOPAGE 792
.OPTION NOPIV 569
.OPTION NOTOP 570
.OPTION NOWARN 571
.OPTION NUMDGT 572
.OPTION NUMERICAL_DERIVATIVES 573
.OPTION NXX 574
.OPTION OFF 575
.OPTION OPFILE 576
Index
O
.OPTION OPTCON 577
.OPTION OPTLST 579
.OPTION OPTS 581
.OPTION PARHIER 582
.OPTION PATHNUM 583, 588
.OPTION PHASENOISEAMPM 593
.OPTION PHASENOISEKRYLOVDIM 586
.OPTION PHASENOISEKRYLOVITER 587
.OPTION PHD 591
.OPTION PHNOISELORENTZ 592
.OPTION PIVOT 594
.OPTION PIVREF 791
.OPTION PIVREL 793
.OPTION PIVTOL 595
.OPTION PLIM 794
.OPTION POST 596
.OPTION POST_VERSION 599
.OPTION POSTLVL 598
.OPTION POSTTOP 601
.OPTION PROBE 602
.OPTION PSF 603
.OPTION PURETP 604
.OPTION PUTMEAS 605
.OPTION PZABS 606
.OPTION PZTOL 607
.OPTION RANDGEN 610
.OPTION RELH 612
.OPTION RELI 613
.OPTION RELMOS 615
.OPTION RELQ 616
.OPTION RELTOL 617
.OPTION RELV 618
.OPTION RELVAR 619
.OPTION RELVDC 620
.OPTION RESMIN 623
.OPTION RISETIME 624
.OPTION RITOL 626
.OPTION RMAX 627
.OPTION RMIN 628
.OPTION RUNLVL 629
N value effect on other options 804
.OPTION SAVEHB 635
.OPTION SAVESNINIT 636
.OPTION SCALE 637
.OPTION SCALM 638
.OPTION SDA 795
.OPTION SEARCH 639
.OPTION SEED 640
.OPTION SIM_ACCURACY 642
.OPTION SIM_DELTAI 643
.OPTION SIM_DELTAV 644
.OPTION SIM_DSPF 645
.OPTION SIM_DSPF_ACTIVE 647
.OPTION SIM_DSPF_INSERROR 648
.OPTION SIM_DSPF_LUMPCAPS 649
.OPTION SIM_DSPF_MAX_ITER 650
.OPTION SIM_DSPF_RAIL 651
.OPTION SIM_DSPF_SCALEC 652
.OPTION SIM_DSPF_SCALER 653
.OPTION SIM_DSPF_VTOL 654
.OPTION SIM_LA 656
.OPTION SIM_LA_FREQ 657
.OPTION SIM_LA_MAXR 658
.OPTION SIM_LA_MINC 659
.OPTION SIM_LA_MINMODE 797
.OPTION SIM_LA_TIME 660
.OPTION SIM_LA_TOL 661
.OPTION SIM_ORDER 662
.OPTION SIM_OSC_DETECT_TOL 663
.OPTION SIM_POSTAT 664
.OPTION SIM_POSTDOWN 665
.OPTION SIM_POSTSCOPE 666
.OPTION SIM_POSTSKIP 667
.OPTION SIM_POSTTOP 668
.OPTION SIM_POWER_ANALYSIS 669
.OPTION SIM_POWER_TOP 670
.OPTION SIM_POWERDC_ACCURACY 671
.OPTION SIM_POWERDC_HSPICE 672
.OPTION SIM_POWERPOST 673
.OPTION SIM_POWERSTART 674
.OPTION SIM_POWERSTOP 675
.OPTION SIM_SPEF 676
.OPTION SIM_SPEF_ACTIVE 677
.OPTION SIM_SPEF_INSERROR 678
.OPTION SIM_SPEF_LUMPCAPS 679
.OPTION SIM_SPEF_MAX_ITER 680
.OPTION SIM_SPEF_PARVALUE 681
.OPTION SIM_SPEF_RAIL 682
.OPTION SIM_SPEF_SCALEC 683
.OPTION SIM_SPEF_SCALER 684
821
Index
P
.OPTION SIM_SPEF_VTOL 685
.OPTION SIM_TG_THETA 686
.OPTION SIM_TRAP 687
.OPTION SLOPETOL 689
.OPTION SNACCURACY 690
.OPTION SNCONTINUE 691
.OPTION SNMAXITER 692
.OPTION SPMODEL 696
.OPTION STATFL 697
.OPTION SYMB 700
.OPTION TIMERES 701
.OPTION TMIFLAG 702
.OPTION TNOM 705
.OPTION TRANFORHB 706
.OPTION TRCON 707
.OPTION TRTOL 708
.OPTION UNWRAP 709
.OPTION VAMODEL 710
.OPTION VERIFY 711
.OPTION VFLOOR 712
.OPTION VNTOL 713
.OPTION WACC 714
.OPTION WARNLIMIT 717
.OPTION WDELAYOPT 719
.OPTION WDF 720
.OPTION WINCLUDEGDIMAG 722
.OPTION WL 723
.OPTION WNFLAG 724
.OPTION XDTEMP 725
.OPTION ZUKEN 798
options
BDFATOL 388, 390
BISACC 354
CAPTAB 404
IVTH 513
MOSRALIFE 554
MOSRASORT 555
NCFILTERr 562
PHD 591
TMIFLAG 702
WDF 720
OPTLST option 579
OPTS option 581
Opus 783, 795
oscillation, eliminating 546
822
oscillator analysis 129, 246
OUT, OUTZ command 742
Output 18
output
ASCII 12
data
format 539, 603
limiting 503
significant digits specification 572
specifying 522
storing 544
data, redirecting 9
files
reducing size of 717
version number, specifying 3, 12
.MEASURE results 171
plotting 777–778
printing 253–??
printout format 501
redirecting 9, 12
variables
printing 512
probing 255
specifying significant digits for 572
ovari 295
P
.PARAM command 237
parameters
ABSOUT optimization bisection 216
AC sweep 25
DC sweep 71
defaults 582
FROM 196
IC 80
inheritance 582
ITROPT optimization 216
matrix 775
names
.MODEL command parameter name 215
simulator access 151
skew, assigning 152
UIC 80, 138
PARHIER option 582
PARMIN optimization parameter 216
.PAT command 241
path names 583
path numbers, printing 583
Index
R
PATHNUM option 583, 588
p-channel
JFETs models 214
MOSFET’s models 214
peak-to-peak value
measuring 187
PERIOD command 743
PERIOD statement 743
periodic pime-dependent noise analysis 261
.PHASENOISE command 244
PHASENOISEAMPM option 593
PHASENOISEKRYLOVDIM option 586
PHASENOISEKRYLOVITER option 587
PHNOISELORENTZ option 592
pivot
algorithm, selecting 594
reference 791
PIVOT option 594
pivot option 594
PIVREF option 791
PIVREL option 793
PIVTOL option 595
.PKG command 247
PLIM option 794
plot
models 214
value calculation method 361
.PLOT command 777
in .ALTER block 33
pnp BJT models 214
POI keyword 26, 72, 316
pole-zero
(X0R, X0I) option 727
(X1R, X1I) option 728
(X2R, X2I) option 729
CSCAL option 414, 529
FSCAL option 460
GSCAL option 469
PZABS option 606
PZTOL option 607
RITOL option 626
pole-zero analysis
FMAX option 458
maximum iterations 511
polygon, defining 275
POST option 596
POST_VERSION option 599
POSTLVL option 598
POSTTOP option 601
.POWER command 249
power operating point table 233
.POWERDC command 251
power-dependent S parameter extraction 122
PP 187, 191
PP keyword 187, 199
.PRINT command 252
in .ALTER 33
printing
Jacobian data 579
printout
disabling 400, 574
suppressing 258
value calculation method 361
.PROBE command 255
PROBE option 602
propogation delays
measuring 175
with .MEASURE 173
.PROTECT command 258
protecting data 258
PSF option 603
PTDNOISE
overview 261
.PTDNOISE command 259
PTDNOISE with .MEASURE command 202
PURETP option 604
pushout bisection 203
PUTMEAS option 605
.PZ command 263
PZABS option 606
PZTOL option 607
R
RADIX scommand 744
RANDGEN option 610
reference temperature 309
RELH option 612
RELI option 514, 613
RELIN optimization parameter 216
RELMOS option 355, 514, 615
RELOUT optimization parameter 216
RELQ option 616
823
Index
S
RELTOL option 406
RELTOLoption 617
RELV option 455, 537, 618
RELVAR option 619
RELVDC option 620
resistance 623
RESMIN option 623
RESULTS keyword 72
RF
.MEASURE PTDNOISE 202
RF commands
.SNNOISE 279, 283
RIN keyword 775
Rise 173
rise and fall times 175
RISE keyword 179, 183
rise time
example 56
specify 749, 751
verify 56
RISETIME option 624
RITOL option 626
RMAX option 627
RMIN option 628
RMS keyword 187, 199
ROUT keyword 775
row/matrix ratio 793
RUNLVL option 629
N value effect on other options 804
S
.SAMPLE 265
.SAMPLE command 265
sampling noise 265
.SAVE command 266
SAVEHB option 635
SAVESNINIT option 636
SCALE option 637
SCALM option 638
SDA option 795
SEARCH option 639
SEED option 640
.SENS command 268
Setup 18
.SHAPE command 270
824
Defining Circles 272
Defining Polygons 273
Defining Rectangles 271
Defining Strip Polygons 275
Shooting Newton syntaxes 277
significant digits 539
SIM_ACCURACY option 642
SIM_DSPF option 645
SIM_DSPF_ACTIVE option 647
SIM_DSPF_DELTAI option 643
SIM_DSPF_DELTAV option 644
SIM_DSPF_INSERROR option 648
SIM_DSPF_LUMPCAPS option 649
SIM_DSPF_MAX_ITER option 650
SIM_DSPF_RAIL option 651
SIM_DSPF_SCALEC option 652
SIM_DSPF_SCALER option 653
SIM_DSPF_VTOL option 654
SIM_LA option 656
SIM_LA_FREQ option 657
SIM_LA_MAXR option 658
SIM_LA_MINC option 659
SIM_LA_MINMODE option 797
SIM_LA_TIME option 660
SIM_LA_TOL option 661
SIM_ORDER option 662
SIM_OSC_DETECT_TOL option 663
SIM_POSTAT option 664
SIM_POSTDOWN option 665
SIM_POSTSCOPE option 666
SIM_POSTSKIP option 667
SIM_POSTTOP option 668
SIM_POWER_ANALYSIS option 669
SIM_POWER_TOP option 670
SIM_POWERDC_ACCURACY option 671
SIM_POWERDC_HSPICE option 672
SIM_POWERPOST option 673
SIM_POWERSTART option 674
SIM_POWERSTOP option 675
SIM_SPEF option 676
SIM_SPEF_ACTIVE option 677
SIM_SPEF_INSERROR option 678
SIM_SPEF_LUMPCAPS option 679
SIM_SPEF_MAX_ITER option 680
SIM_SPEF_PARVALUE option 681
Index
S
SIM_SPEF_RAIL option 682
SIM_SPEF_SCALEC option 683
SIM_SPEF_SCALER option 684
SIM_SPEF_VTOL option 685
SIM_TG_THETA option 686
SIM_TG_TRAP option 687
simulation
accuracy 360, 531
accuracy improvement 448
multiple analyses, .ALTER command 33
multiple runs 94
reducing time 65, 368, 448, 500, 507, 689, 708
results
plotting 777–778
printing 253
specifying 171
title 313
Simulation Runs 18
skew, parameters 152
slew rate
verification 59
SLEW, .CHECK command 59
SLOPE command 745
SLOPETOL option 689
small-signal, DC sensitivity 268
.SN command 277
SNACCURACY option 690
SNCONTINUE option 691
.SNFT command 280
SNMAXITER option 692
.SNNOISE command 279, 283
.SNOSC command 285
.SNXF command 288
source
AC sweep 25
DC sweep 71
S-parameter, model type 214
SPICE
compatibility
AC output 361
plot 794
SPMODEL option 696
START keyword 315
statements
.AC 25
.ACMATCH 28
.ALIAS 31
.ALTER 33, 81
alter block 15
.BIASCHK 38
.CHECK EDGE 48
.CHECK FALL 50
.CHECK GLOBAL_LEVEL 51
.CHECK HOLD 52
.CHECK IRDROP 54
.CHECK RISE 56
.CHECK SETUP 58
.CHECK SLEW 59
.CONNECT 61
.DATA 64
external file 64
inline 64
.DC 71, 73
.DCMATCH 76
.DCVOLT 80, 138
.DEL LIB 81
.DISTO 86, 87
.DOUT 88
.EBD 90
.ELSE 92
.ELSEIF 93
.END 94
.ENDDATA 95
.ENDIF 96
.ENDL 97, 151
.ENDS 98, 102
.ENV 99
.ENVFFT 100
.ENVOSC 101
.EOM 102
.FFT 103
.FOUR 110
.FSOPTIONS 111
.GLOBAL 114
.GRAPH 771
.HB 115
.HBAC 118
.HBLIN 119
.HBLSP 121
.HBNOISE 123
.HBOSC 126
.HBXF 131
.HDL 132
.IBIS 134
.IC 80, 138
825
Index
T
.ICM 140
.IF 142
.INCLUDE 92, 94, 142, 144, 267
.LAYERSTACK 148
.LIB 150, 151
nesting 151
.LIN 154
.LOAD 158
.LPRINT 160
.MACRO 164
.MALIAS 167
.MATERIAL 169
.MEASURE 171, 539, 544
.MODEL 213
.MOSRA 222
.MOSRAPRINT 226
.NET 775
.NODESET 228
.NOISE 230
.OP 233, 234
.PARAM 237
.PAT 241
.PERIOD 743
.PHASENOISE 244
.PKG 247
.PLOT 777
.POWER 249
.POWERDC 251
.PRINT 252
.PROBE 255
.PROTECT 258
.PZ 263
.SAMPLE 265
.SAVE 266
.SENS 268
.SHAPE 270
.SNFT 280
.SNOSC 285
.SNXF 288
.STIM 294
.SUBCKT 301
.SURGE 306
.SWEEPBLOCK 307
.TEMP 309
.TF 312
.TITLE 313
.TRAN 314
.UNPROTECT 324
826
.VARIATION 325
.VEC 327
.WIDTH 779
.STATEYE command 290
STATFL option 697
statistical eye diagram analysis 290
statistics, listing 780
.STIM command 294
subcircuit commands 18
subcircuits
calling 165, 302
global versus local nodes 114
names 164, 301
node numbers 164, 301
parameter 98, 102, 164, 165, 301, 302
printing path numbers 583
.SUBCKT command 301
.SURGE command 306
sweep
data 544
frequency 27
SWEEP keyword 26, 72, 315
.SWEEPBLOCK command 307
SYMB option 700
T
Tabular Data section
time interval 743
TARG_SPEC 173
target specification 173, 182
TDELAY command 747
TEMP
keyword 26, 72
model parameter 309
.TEMP (or) .TEMPERATURE command 309
temperature
AC sweep 25
DC sweep 71
derating 309, 310
reference 309
.TF command 312
TFALL command 749
TIC model parameter 773
time 233
See also CPU time
TIMERES option 701
timestep
Index
U
algorithms 448
calculation for DVDT=3 459
changing size 616
control 459, 619, 708
maximum 499, 508, 627
minimum 500, 507, 628
reversal 358
transient analysis algorithm 531
.TITLE command 313
title for simulation 313
TMI flow 702
TNOM option 309, 705
TO keyword 188, 191, 197
TOL keyword 265
TOP keyword 266
.TRAN command 314
TRANFORHB option 706
transient analysis
Fourier analysis 110
initial conditions 80, 138
number of iterations 509
TRAP algorithm
See trapezoidal integration
TRCON option 707
TRIG keyword 173
TRIG_SPEC 173
trigger specification 173, 182
TRISE command 749, 751
TRIZ command 753
TRTOL option 708
TSKIP command 754
TSTEP
multiplier 627, 628
option 627, 628
TUNIT command 755
U
UIC
parameter 80, 138
U-lement, transmission line model 214
.UNPROTECT command 324
UNWRAP option 709
V
-v argument
version information 12
VAMODEL option 710
.VARIATION command 325
.VEC command 327
VEC commands
ENABLE 736
IDELAY 737
IO 739
ODELAY 740
OUT, OUTZ 742
PERIOD 743
RADIX 744
SLOPE 745
TDELAY 747
TFALL 749
TRISE 751
TRIZ 753
TSKIP 754
TUNIT 755
VIH 757
VIL 758
VNAME 759
VOH 761
VOL 763
VREF 765
VTH 766
VERIFY option 711
Verilog-A commands 19
version
determining 12
H9007 compatibility 786
VFLOOR option 712
Viewlogic graph data file 446
VIH command 757
VIL command 758
VNAME command 759
VNTOL option 455, 713
VOH command 761, 763
VOL command 763
voltage
initial conditions 80, 138
iteration-to-iteration change 447
logic high 757, 761
logic low 758
logic low threshold 763
maximum change 358
minimum
DC analysis 359
listing 712
827
Index
W
transient analysis 357
operating point table 233
tolerance
MBYPASS multiplier 537
value for BYPASS 403
VOLTAGE keyword 233
VREF command 765
VREF statement 765
VTH command 766
W
WACC option 714
warnings
limiting repetitions 717
suppressing 571
WARNLIMIT option 717
WDELAYOPT option 719
WEIGHT keyword 188, 196
W-elements transmission line model 214
WHEN keyword 180
WHEN, using with .MEASURE 178
.WIDTH command 779
WINCLUDEGDIMAG option 722
828
WL option 723
WNFLAG option 724
WSF output data 783, 795
X
XDTEMP option 725
XGRID model parameter 773
XMAX model parameter 773
XMIN model parameter 773
XSCAL model parameter 773
Y
YGRID model parameter 773
YMAX parameter 196, 773
YMIN parameter 196, 773
YSCAL model parameter 774
Z
ZUKEN option 798
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement