HSPICE Command Reference - Electrical and Computer Engineering

HSPICE Command Reference - Electrical and Computer Engineering
HSPICE® Command Reference
Version X-2005.09, September 2005
Copyright Notice and Proprietary Information
Copyright  2005 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, Arcadia, C Level Design, C2HDL, C2V, C2VHDL, Cadabra, Calaveras Algorithm, CATS, CRITIC,
CSim, Design Compiler, DesignPower, DesignWare, EPIC, Formality, HSIM, HSPICE, Hypermodel, iN-Phase, in-Sync,
Leda, MAST, Meta, Meta-Software, ModelTools, NanoSim, OpenVera, PathMill, Photolynx, Physical Compiler, PowerMill,
PrimeTime, RailMill, RapidScript, Saber, SiVL, SNUG, SolvNet, Superlog, System Compiler, Testify, TetraMAX, TimeMill,
TMA, VCS, Vera, and Virtual Stepper are registered trademarks of Synopsys, Inc.
Trademarks (™)
Active Parasitics, AFGen, Apollo, Apollo II, Apollo-DPII, Apollo-GA, ApolloGAII, Astro, Astro-Rail, Astro-Xtalk, Aurora,
AvanTestchip, AvanWaves, BCView, Behavioral Compiler, BOA, BRT, Cedar, ChipPlanner, Circuit Analysis, Columbia,
Columbia-CE, Comet 3D, Cosmos, CosmosEnterprise, CosmosLE, CosmosScope, CosmosSE, Cyclelink, Davinci, DC
Expert, DC Expert Plus, DC Professional, DC Ultra, DC Ultra Plus, Design Advisor, Design Analyzer, Design Vision,
DesignerHDL, DesignTime, DFM-Workbench, Direct RTL, Direct Silicon Access, Discovery, DW8051, DWPCI,
Dynamic-Macromodeling, Dynamic Model Switcher, ECL Compiler, ECO Compiler, EDAnavigator, Encore, Encore PQ,
Evaccess, ExpressModel, Floorplan Manager, Formal Model Checker, FoundryModel, FPGA Compiler II, FPGA Express,
Frame Compiler, Galaxy, Gatran, HANEX, HDL Advisor, HDL Compiler, Hercules, Hercules-Explorer, Hercules-II,
Hierarchical Optimization Technology, High Performance Option, HotPlace, HSIMplus, HSPICE-Link, iN-Tandem,
Integrator, Interactive Waveform Viewer, i-Virtual Stepper, Jupiter, Jupiter-DP, JupiterXT, JupiterXT-ASIC, JVXtreme,
Liberty, Libra-Passport, Library Compiler, Libra-Visa, Magellan, Mars, Mars-Rail, Mars-Xtalk, Medici, Metacapture,
Metacircuit, Metamanager, Metamixsim, Milkyway, ModelSource, Module Compiler, MS-3200, MS-3400, Nova Product
Family, Nova-ExploreRTL, Nova-Trans, Nova-VeriLint, Nova-VHDLlint, Optimum Silicon, Orion_ec, Parasitic View,
Passport, Planet, Planet-PL, Planet-RTL, Polaris, Polaris-CBS, Polaris-MT, Power Compiler, PowerCODE, PowerGate,
ProFPGA, ProGen, Prospector, Protocol Compiler, PSMGen, Raphael, Raphael-NES, RoadRunner, RTL Analyzer,
Saturn, ScanBand, Schematic Compiler, Scirocco, Scirocco-i, Shadow Debugger, Silicon Blueprint, Silicon Early Access,
SinglePass-SoC, Smart Extraction, SmartLicense, SmartModel Library, Softwire, Source-Level Design, Star, Star-DC,
Star-MS, Star-MTB, Star-Power, Star-Rail, Star-RC, Star-RCXT, Star-Sim, Star-SimXT, Star-Time, Star-XP, SWIFT,
Taurus, TimeSlice, TimeTracker, Timing Annotator, TopoPlace, TopoRoute, Trace-On-Demand, True-Hspice,
TSUPREM-4, TymeWare, VCS Express, VCSi, Venus, Verification Portal, VFormal, VHDL Compiler, VHDL System
Simulator, 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.
All other product or company names may be trademarks of their respective owners.
Printed in the U.S.A.
HSPICE® Command Reference, X-2005.09
ii
HSPICE® Command Reference
X-2005.09
Contents
1.
Inside This Manual. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xv
The HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xvi
Searching Across the HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . .
xvii
Other Related Publications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xvii
Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xviii
Customer Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xix
Command Categories . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1
Alter Blocks . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1
Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1
Conditional Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2
Digital Vector . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2
Encryption . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2
Field Solver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3
Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3
Input/Output Buffer Information Specification (IBIS) . . . . . . . . . . . . . . . . . . . .
3
Library Management . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3
Model Definition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4
Node Naming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4
Output Porting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4
Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4
Simulation Runs. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5
Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5
Verilog-A . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5
HSPICE® Command Reference
X-2005.09
iii
Contents
2.
iv
Commands in HSPICE Netlists. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7
.AC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9
.ALIAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14
.ALTER. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
.BIASCHK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
.CONNECT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
23
.DATA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
25
.DC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
32
.DCMATCH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
38
.DCVOLT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
40
.DEL LIB. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
42
.DISTO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
46
.DOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
49
.EBD. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
52
.ELSE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
54
.ELSEIF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
55
.END . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
56
.ENDDATA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
57
.ENDIF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
58
.ENDL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
59
.ENDS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
60
.EOM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
61
.FFT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
62
.FOUR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
65
.FSOPTIONS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
66
.GLOBAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
68
.GRAPH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
69
.HDL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
71
.IBIS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
72
.IC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
76
HSPICE® Command Reference
X-2005.09
Contents
.ICM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
78
.IF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
79
.INCLUDE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
81
.LAYERSTACK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
82
.LIB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
84
.LIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
88
.LOAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
91
.MACRO. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
93
.MALIAS. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
96
.MATERIAL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
98
.MEASURE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
100
.MEASURE (Rise, Fall, and Delay Measurements) . . . . . . . . . . . . . . . . . . . . .
101
.MEASURE (Average, RMS, and Peak Measurements) . . . . . . . . . . . . . . . . .
105
.MEASURE (FIND and WHEN) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
107
.MEASURE (Equation Evaluation/ Arithmetic Expression) . . . . . . . . . . . . . . .
111
.MEASURE (Average, RMS, MIN, MAX, INTEG, and PP). . . . . . . . . . . . . . . .
112
.MEASURE (Integral Function) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
115
.MEASURE (Derivative Function) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
116
.MEASURE (Error Function) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
119
.MEASURE (Pushout Bisection) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
121
.MODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
123
.NET. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
129
.NODESET. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
131
.NOISE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
132
.OP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
133
.OPTION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
135
.PARAM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
137
.PAT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
141
.PKG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
143
.PLOT. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
145
.PRINT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
147
HSPICE® Command Reference
X-2005.09
v
Contents
3.
vi
.PROBE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
151
.PROTECT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
153
.PZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
154
.SAMPLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
156
.SAVE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
157
.SENS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
159
.SHAPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
161
.SHAPE (Defining Rectangles) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
162
.SHAPE (Defining Circles) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
163
.SHAPE (Defining Polygons) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
164
.SHAPE (Defining Strip Polygons) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
166
.STIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
167
.SUBCKT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
172
.TEMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
175
.TF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
177
.TITLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
178
.TRAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
179
.UNPROTECT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
184
.VEC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
185
.WIDTH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
186
Options in HSPICE Netlists. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
187
General Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
188
CPU Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
188
Interface Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
188
Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
189
Error Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
189
Version Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
189
Model Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
189
General Model Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
189
MOSFET Model Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
189
HSPICE® Command Reference
X-2005.09
Contents
Inductor Model Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
190
BJT and Diode Model Analysis Options. . . . . . . . . . . . . . . . . . . . . . . . . .
190
DC Operating Point, DC Sweep, and Pole/Zero Options . . . . . . . . . . . . . . . . .
190
DC Accuracy Options. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
190
DC Matrix Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
190
DC Pole/Zero I/O Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
190
DC Convergence Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
191
DC Initialization Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
191
Transient and AC Small Signal Analysis Options. . . . . . . . . . . . . . . . . . . . . . .
191
Transient/AC Accuracy Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
191
Transient/AC Speed Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
192
Transient/AC Timestep Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
192
Transient/AC Algorithm Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
192
.BIASCHK Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
192
Transient Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
193
Transient Control Method Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
193
Transient Control Tolerance Options . . . . . . . . . . . . . . . . . . . . . . . . . . . .
193
Transient Control Limit Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
193
Transient Control Matrix Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
194
Iteration Count Dynamic Timestep Options . . . . . . . . . . . . . . . . . . . . . . .
194
Input/Output Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
194
AC Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
194
Common Model Interface Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
194
Verilog-A Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
194
.OPTION ABSH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
195
.OPTION ABSI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
196
.OPTION ABSMOS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
197
.OPTION ABSTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
198
.OPTION ABSV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
199
.OPTION ABSVAR. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
200
.OPTION ABSVDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
201
.OPTION ACCT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
202
.OPTION ACCURATE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
203
.OPTION ACOUT. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
204
HSPICE® Command Reference
X-2005.09
vii
Contents
viii
.OPTION ALT999 or ALT9999 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
205
OPTION ALTCC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
206
.OPTION ALTCHK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
207
.OPTION ARTIST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
208
.OPTION ASPEC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
209
.OPTION AUTOSTOP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
210
.OPTION BADCHR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
211
.OPTION BEEP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
212
.OPTION BIASFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
213
.OPTION BIAWARN. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
214
.OPTION BINPRINT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
215
.OPTION BKPSIZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
216
.OPTION BRIEF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
217
.OPTION BYPASS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
218
.OPTION BYTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
219
.OPTION CAPTAB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
220
.OPTION CDS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
221
.OPTION CHGTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
222
.OPTION CMIFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
223
.OPTION CO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
224
.OPTION CONVERGE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
225
.OPTION CPTIME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
226
.OPTION CSDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
227
.OPTION CSHDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
228
.OPTION CSHUNT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
229
.OPTION CUSTCMI. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
230
.OPTION CVTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
231
.OPTION D_IBIS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
232
.OPTION DCAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
233
.OPTION DCCAP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
234
.OPTION DCFOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
235
HSPICE® Command Reference
X-2005.09
Contents
.OPTION DCHOLD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
236
.OPTION DCIC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
237
.OPTION DCON. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
238
.OPTION DCSTEP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
239
.OPTION DCTRAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
240
.OPTION DEFAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
241
.OPTION DEFAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
242
.OPTION DEFL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
243
.OPTION DEFNRD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
244
.OPTION DEFNRS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
245
.OPTION DEFPD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
246
.OPTION DEFPS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
247
.OPTION DEFW. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
248
.OPTION DELMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
249
.OPTION DI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
250
.OPTION DIAGNOSTIC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
251
.OPTION DLENCSDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
252
.OPTION DV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
253
.OPTION DVDT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
254
.OPTION DVTR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
255
.OPTION EPSMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
256
.OPTION EXPLI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
257
.OPTION EXPMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
258
.OPTION FAST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
259
.OPTION FFTOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
260
.OPTION FS. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
261
.OPTION FT. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
262
.OPTION GDCPATH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
263
.OPTION GENK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
264
.OPTION GMAX. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
265
.OPTION GMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
266
HSPICE® Command Reference
X-2005.09
ix
Contents
x
.OPTION GMINDC. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
267
.OPTION GRAMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
268
.OPTION GSHDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
269
.OPTION GSHUNT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
270
.OPTION H9007. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
271
.OPTION HIER_SCALE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
272
.OPTION ICSWEEP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
273
.OPTION IMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
274
.OPTION IMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
275
.OPTION INGOLD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
276
.OPTION INTERP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
277
.OPTION ITL1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
278
.OPTION ITL2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
279
.OPTION ITL3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
280
.OPTION ITL4 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
281
.OPTION ITL5 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
282
.OPTION ITLPTRAN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
283
.OPTION ITLPZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
284
.OPTION ITRPRT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
285
.OPTION KCLTEST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
286
.OPTION KLIM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
287
.OPTION LENNAM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
288
.OPTION LIMPTS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
289
.OPTION LIMTIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
290
.OPTION LIST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
291
.OPTION LVLTIM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
292
.OPTION MAXAMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
293
.OPTION MAXORD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
294
.OPTION MBYPASS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
295
.OPTION MCBRIEF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
296
.OPTION MEASDGT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
297
HSPICE® Command Reference
X-2005.09
Contents
.OPTION MEASFAIL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
298
.OPTION MEASFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
299
.OPTION MEASSORT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
300
.OPTION MEASOUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
301
.OPTION MENTOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
302
.OPTION METHOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
303
.OPTION MODMONTE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
304
.OPTION MODSRH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
305
.OPTION MONTECON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
306
.OPTION MU . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
307
.OPTION NEWTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
308
.OPTION NODE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
309
.OPTION NOELCK . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
310
.OPTION NOISEMINFREQ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
311
.OPTION NOMOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
312
.OPTION NOPAGE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
313
.OPTION NOPIV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
314
.OPTION NOTOP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
315
.OPTION NOWARN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
316
.OPTION NUMDGT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
317
.OPTION NXX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
318
.OPTION OFF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
319
.OPTION OPFILE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
320
.OPTION OPTLST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
321
.OPTION OPTS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
322
.OPTION PARHIER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
323
.OPTION PATHNUM . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
324
.OPTION PIVOT. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
325
.OPTION PIVREF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
327
.OPTION PIVREL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
328
.OPTION PIVTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
329
HSPICE® Command Reference
X-2005.09
xi
Contents
xii
.OPTION PLIM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
330
.OPTION POST . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
331
.OPTION POSTLVL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
332
.OPTION POST_VERSION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
333
.OPTION POSTTOP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
334
.OPTION PROBE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
335
.OPTION PSF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
336
.OPTION PURETP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
337
.OPTION PUTMEAS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
338
.OPTION RELH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
339
.OPTION RELI . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
340
.OPTION RELMOS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
341
.OPTION RELQ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
342
.OPTION RELTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
343
.OPTION RELV . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
344
.OPTION RELVAR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
345
.OPTION RELVDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
346
.OPTION RESMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
347
.OPTION RISETIME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
348
.OPTION RMAX. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
349
.OPTION RMIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
350
.OPTION RUNLVL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
351
.OPTION SCALE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
353
.OPTION SCALM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
354
.OPTION SDA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
355
.OPTION SEARCH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
356
.OPTION SEED . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
357
.OPTION SLOPETOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
358
.OPTION SPARSE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
359
.OPTION SPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
360
.OPTION SPMODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
361
HSPICE® Command Reference
X-2005.09
Contents
4.
.OPTION STATFL. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
362
.OPTION SYMB . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
363
.OPTION TIMERES . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
364
.OPTION TNOM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
365
.OPTION TRCON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
366
.OPTION TRTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
368
.OPTION UNWRAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
369
.OPTION VAMODEL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
370
.OPTION VERIFY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
371
.OPTION VFLOOR . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
372
.OPTION VNTOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
373
.OPTION WACC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
374
.OPTION WNFLAG . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
375
.OPTION WARNLIMIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
376
.OPTION WL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
377
.OPTION XDTEMP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
378
.OPTION ZUKEN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
379
Commands in Digital Vector Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
393
ENABLE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
394
IDELAY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
395
IO . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
397
ODELAY. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
398
OUT or OUTZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
400
PERIOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
401
RADIX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
402
SLOPE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
403
TDELAY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
404
TFALL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
406
TRISE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
407
TRIZ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
409
HSPICE® Command Reference
X-2005.09
xiii
Contents
xiv
TSKIP. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
410
TUNIT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
411
VIH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
412
VIL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
413
VNAME . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
414
VOH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
416
VOL . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
418
VREF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
420
VTH . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
421
Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
423
HSPICE® Command Reference
X-2005.09
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, Command
Categories
Lists all commands you can use in HSPICE,
arranged by task.
Chapter 2, Commands in
HSPICE Netlists
Contains an alphabetical listing of all commands
you can use in an HSPICE netlist.
Chapter 3, Options in
HSPICE Netlists
Describes the simulation options you can set
using various forms of the .OPTION command.
Chapter 4, Commands in
Digital Vector Files
Contains an alphabetical listing of the commands
you can use in an digital vector file.
HSPICE® Command Reference
X-2005.09
xv
About This Manual
The HSPICE Documentation Set
The HSPICE Documentation Set
This manual is a part of the HSPICE documentation set, which includes the
following manuals:
xvi
Manual
Description
HSPICE Simulation and
Analysis User Guide
Describes how to use HSPICE to simulate and
analyze your circuit designs. This is the main
HSPICE user guide.
HSPICE Signal Integrity
Guide
Describes how to use HSPICE to maintain signal
integrity in your chip design.
HSPICE Applications
Manual
Provides application examples and additional
HSPICE user information.
HSPICE Command
Reference
Provides reference information for HSPICE
commands.
HPSPICE Elements and
Device Models Manual
Describes standard models you can use when
simulating your circuit designs in HSPICE,
including passive devices, diodes, JFET and
MESFET devices, and BJT devices.
HPSPICE MOSFET Models
Manual
Describes standard MOSFET models you can
use when simulating your circuit designs in
HSPICE.
HSPICE RF Manual
Describes a special set of analysis and design
capabilities added to HSPICE to support RF and
high-speed circuit design.
AvanWaves User Guide
Describes the AvanWaves tool, which you can
use to display waveforms generated during
HSPICE circuit design simulation.
HSPICE® Command Reference
X-2005.09
About This Manual
Searching Across the HSPICE Documentation Set
Manual
Description
HSPICE Quick Reference
Guide
Provides key reference information for using
HSPICE, including syntax and descriptions for
commands, options, parameters, elements, and
more.
HSPICE Device Models
Quick Reference Guide
Provides key reference information for using
HSPICE device models, including passive
devices, diodes, JFET and MESFET devices,
and BJT devices.
Searching Across the HSPICE Documentation Set
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 (available on SolvNet at http://solvnet.synopsys.com) or the Adobe
Reader online help.
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.
Other Related Publications
For additional information about HSPICE, see:
■
The HSPICE release notes, available on SolvNet (see Accessing SolvNet
on page xix)
■
Documentation on the Web, which provides PDF documents and is
available through SolvNet at http://solvnet.synopsys.com
■
The Synopsys MediaDocs Shop, from which you can order printed copies
of Synopsys documents, at http://mediadocs.synopsys.com
HSPICE® Command Reference
X-2005.09
xvii
About This Manual
Conventions
You might also want to refer to the documentation for the following related
Synopsys products:
■
CosmosScope
■
Aurora
■
Raphael
■
VCS
Conventions
The following conventions are used in Synopsys documentation:
Convention
Description
Courier
Indicates command syntax.
Italic
Indicates a user-defined value, such as object_name.
Bold
Indicates user input—text you type verbatim—in syntax and
examples.
[]
Denotes optional parameters, such as
write_file [-f filename]
...
Indicates that a parameter can be repeated as many times
as necessary:
pin1 [pin2 ... pinN]
|
Indicates a choice among alternatives, such as
low | medium | high
xviii
\
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.
HSPICE® Command Reference
X-2005.09
About This Manual
Customer Support
Customer Support
Customer support is available through SolvNet online customer support and
through contacting the Synopsys Technical Support Center.
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 SolvNet Help in the Support Resources
section.
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 (Synopsys user name and password required),
then clicking “Enter a Call to the Support Center.”
■
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.
HSPICE® Command Reference
X-2005.09
xix
About This Manual
Customer Support
•
■
xx
Call (650) 584-4200 from Canada.
Find other local support center telephone numbers at
http://www.synopsys.com/support/support_ctr.
HSPICE® Command Reference
X-2005.09
1
Command Categories
1
Lists all commands you can use in HSPICE, arranged by task.
Alter Blocks
Use these commands in your HSPICE netlist to run alternative simulations of
your netlist by using different data.
.ALIAS
.ALTER
.DEL LIB
.TEMP
Analysis
Use these commands in your HSPICE 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.
.AC
.LIN
.SAMPLE
.DC
.NET
.SENS
.DCMATCH
.NOISE
.TEMP
HSPICE® Command Reference
X-2005.09
1
1: Command Categories
Conditional Block
.DISTO
.OP
.TF
.FFT
.PAT
.TRAN
.FOUR
.PZ
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
.IF
Digital Vector
Use these commands in your digital vector (VEC) file.
ENABLE
SLOPE
VIH
IDELAY
TDELAY
VIL
IO
TFALL
VNAME
ODELAY
TRISE
VOH
OUT or OUTZ
TRIZ
VOL
PERIOD
TSKIP
VREF
RADIX
TUNIT
VTH
Encryption
Use these commands in your HSPICE netlist to mark the start and end of an
encrypted section of a netlist.
.PROTECT
2
.UNPROTECT
HSPICE® Command Reference
X-2005.09
1: Command Categories
Field Solver
Field Solver
Use these commands in your HSPICE netlist to define a field solver.
.FSOPTIONS
.LAYERSTACK
.MATERIAL
.SHAPE
Files
Use this command in your HSPICE netlist to call other files that are not part of
the netlist.
.VEC
Input/Output Buffer Information Specification (IBIS)
Use these commands in your HSPICE netlist for specifying input/output buffer
information.
.EBD
.IBIS
.ICM
.PKG
Library Management
Use these commands in your HSPICE netlist to manage libraries of circuit
designs, and to call other files when simulating your netlist.
3
.DEL LIB
.INCLUDE
.PROTECT
.ENDL
.LIB
.UNPROTECT
HSPICE® Command Reference
X-2005.09
1: Command Categories
Model Definition
Model Definition
Use these commands in your HSPICE netlist to define models.
.MALIAS
.MODEL
Node Naming
Use these commands in your HSPICE netlist to name nodes in circuit designs.
.CONNECT
.GLOBAL
Output Porting
Use these commands in your HSPICE netlist to specify the output of a
simulation to a printer, plotter, or graph. You can also define the parameters to
measure, and to report in the simulation output.
.BIASCHK
.MEASURE
.PROBE
.DOUT
.PLOT
.STIM
.GRAPH
.PRINT
.WIDTH
Setup
Use these commands in your HSPICE netlist to setup your netlist for
simulation.
4
.DATA
.IC
.PARAM
.DCVOLT
.LOAD
.SAVE
.ENDDATA
.NODESET
.TITLE
.GLOBAL
.OPTION
HSPICE® Command Reference
X-2005.09
1: Command Categories
Simulation Runs
Simulation Runs
Use these commands in your HSPICE netlist to mark the start and end of
individual simulation runs, and conditions that apply throughout an individual
simulation run.
.END
.TEMP
.TITLE
Subcircuits
Use these commands in your HSPICE netlist to define subcircuits, and to add
instances of subcircuits to your netlist.
.ENDS
.INCLUDE
.MODEL
.EOM
.MACRO
.SUBCKT
Verilog-A
Use the following command in your HSPICE netlist to declare the Verilog-A
source name and path within the netlist.
.HDL
5
HSPICE® Command Reference
X-2005.09
1: Command Categories
Verilog-A
6
HSPICE® Command Reference
X-2005.09
2
Commands in HSPICE Netlists
2
Contains an alphabetical listing of all commands you can use in an
HSPICE netlist.
Here are the commands described in this chapter. For a list of commands
grouped according to tasks that use each command, see Chapter 1, Command
Categories.
.AC
.FSOPTIONS
.OPTION
.ALIAS
.GLOBAL
.PARAM
.ALTER
.GRAPH
.PAT
.BIASCHK
.HDL
.PKG
.CONNECT
.IBIS
.PLOT
.DATA
.IC
.PRINT
.DC
.ICM
.PROBE
.DCMATCH
.IF
.PROTECT
.DCVOLT
.INCLUDE
.PZ
HSPICE® Command Reference
X-2005.09
7
2: Commands in HSPICE Netlists
.DEL LIB
.LAYERSTACK
.SAMPLE
.DISTO
.LIB
.SAVE
.DOUT
.LIN
.SENS
.EBD
.LOAD
.SHAPE
.ELSE
.MACRO
.STIM
.ELSEIF
.MALIAS
.SUBCKT
.END
.MATERIAL
.TEMP
.ENDDATA
.MEASURE
.TF
.ENDIF
.MODEL
.TITLE
.ENDL
.NET
.TRAN
.ENDS
.NODESET
.UNPROTECT
.EOM
.NOISE
.VEC
.FFT
.OP
.WIDTH
.FOUR
8
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.AC
.AC
Syntax
Single/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_expr1"
+ STOP="param_expr2" STEP="param_expr3">
.AC DATA = datanm <SWEEP var start_expr stop_expr
+ step_expr>
In HSPICE RF, you can run a parameter sweep around a single analysis, but
the parameter sweep cannot change .OPTION values.
Optimization
.AC DATA = datanm OPTIMIZE = opt_par_fun
+ RESULTS = measnames MODEL = optmod
HSPICE RF supports optimization for bisection only.
HSPICE® Command Reference
X-2005.09
9
2: Commands in HSPICE Netlists
.AC
Random/Monte Carlo
.AC type np fstart fstop <SWEEP MONTE = val>
+ <firstrun = num1>
-or.AC type np fstart fstop <SWEEP MONTE = list<(>
+ <num1:num2> <num3> <num5:num6> <num7> <)> >
Example 1
.AC DEC 10 1K 100MEG
This example performs a frequency sweep, by 10 points per decade, from 1kHz
to 100MHz.
Example 2
.AC LIN 100 1 100HZ
This example runs a 100-point frequency sweep from 1- to 100-Hz.
Example 3
.AC DEC 10 1 10K SWEEP cload LIN 20 1pf 10pf
This example performs an AC analysis for each value of cload. This results
from a linear sweep of cload between 1- and 10-pF (20 points), sweeping the
frequency by 10 points per decade, from 1- to 10-kHz.
Example 4
.AC DEC 10 1 10K SWEEP rx POI 2 5k 15k
This example performs an AC analysis for each value of rx, 5k and 15k,
sweeping the frequency by 10 points per decade, from 1- to 10-kHz.
Example 5
.AC DEC 10 1 10K SWEEP DATA = datanm
This example uses the .DATA statement to perform a series of AC analyses,
modifying more than one parameter. The datanm file contains the parameters.
10
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.AC
Example 6
.AC DEC 10 1 10K SWEEP MONTE = 30
This example illustrates a frequency sweep, and a Monte Carlo analysis (not
supported in HSPICE RF) with 30 trials.
Example 7
AC DEC 10 1 10K SWEEP MONTE = 10 firstrun=15
This example illustrates a frequency sweep and a Monte Carlo analysis from
the 15th to the 24th trials.
Example 8
.AC DEC 10 1 10K SWEEP MONTE = list(10 20:30 35:40 50)
This example illustrates a frequency sweep and a Monte Carlo analysis at 10th
trial, and then from the 20th to 30th trial, followed by the 35th to 40th trial, and
finally at 50th trial.
Description
You can use the.AC statement in several different formats, depending on the
application as shown in the examples. You can also use the .AC statement to
perform data-driven analysis in HSPICE.
If the input file includes an .AC statement, 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 statement (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.
You also cannot use this statement in HSPICE RF.
Argument
Definition
DATA =
datanm
Data name, referenced in the .AC statement (not supported in HSPICE
RF).
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.
HSPICE® Command Reference
X-2005.09
11
2: Commands in HSPICE Netlists
.AC
Argument
Definition
fstart
Starting frequency. If you use POI (list of points) type variation, use a
list of frequency values, not fstart fstop.
fstop
Final frequency.
MONTE = val Produces a number (val) of randomly-generated values (HSPICE only;
not supported in HSPICE RF). HSPICE uses these values to select
parameters from a distribution, either Gaussian, Uniform, or Random
Limit.
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
Indicates that the .AC statement specifies a second sweep.
TEMP
Indicates a temperature sweep
type
Can be any of the following keywords:
•
•
•
•
var
12
DEC – decade variation.
OCT – octave variation.
LIN – linear variation.
POI – list of points.
Name of an independent voltage or current source, element or model
parameter, or the TEMP (temperature sweep) keyword. HSPICE or
HSPICE RF supports source value sweep, referring to the source name
(SPICE style). If you select a parameter sweep, a .DATA statement, 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 statement. The
parameter name cannot start with V or I.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.AC
Argument
Definition
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.
See Also
.DC
.TRAN
HSPICE® Command Reference
X-2005.09
13
2: Commands in HSPICE Netlists
.ALIAS
.ALIAS
Syntax
.ALIAS <model_name1> <model_name2>
Example 1
You delete a library named poweramp, that contains a model named pa1.
Another library contains an equivalent model named par1. You can then alias
the pa1 model name to the par1 model name:
.ALIAS pa1 par1
During simulation when HSPICE encounters a model named pa1 in your
netlist, it initially cannot find this model because you used a .ALTER statement
to delete the library that contained the model. However, the .ALIAS statement
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
You also cannot alias a model name to more than one model name, because
then the simulator would not know which of these new models to use in place of
the deleted or renamed model:
.ALIAS pa1 par1 par2
For the same reason, you cannot alias a model name to a second model name,
and then alias the second model name to a third model name:
.ALIAS pa1 par1
.ALIAS par1 par2
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.
14
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.ALIAS
Example 2
Your netlist might contain the statement:
.ALIAS myfet nfet
Without a .ALTER statement, 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.
Description
You can use .ALTER statements 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 statements, HSPICE no longer finds this model.
Note: HSPICE RF does not support the .ALIAS statement.
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 a .ALIAS command to let you alias the
old model name to another model name that HSPICE can find in the existing
model libraries.
See Also
.ALTER
.MALIAS
HSPICE® Command Reference
X-2005.09
15
2: Commands in HSPICE Netlists
.ALTER
.ALTER
Syntax
.ALTER <title_string>
Example
.ALTER simulation_run2
Description
You can use the .ALTER statement to rerun an HSPICE simulation by using
different parameters and data. HSPICE RF does not support the .ALTER
statement.
Use parameter (variable) values for .PRINT and .PLOT statements, before you
alter them. The .ALTER block cannot include .PRINT, .PLOT, .GRAPH or any
other input/output statements. You can include analysis statements
(.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 simulation runs faster if you specify all analysis types in one
block, instead of using separate .ALTER blocks for each analysis type.
The .ALTER sequence or block can contain:
16
■
Element statements (except source elements)
■
.ALIAS statements
■
.DATA statements
■
.DEL LIB statements
■
.IC (initial condition) and .NODESET statements
■
.INCLUDE statements
■
.LIB statements
■
.MODEL statements
■
.OP statements
■
.OPTION statements
■
.PARAM statements
■
.TEMP statements
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.ALTER
■
.TF statements
■
.TRAN, .DC, and .AC statements
Argument
Definition
title_string
Any string up to 72 characters. HSPICE prints the appropriate title
string for each .ALTER run in each section heading of the output
listing, and in the graph data (.tr#) files.
Note: The .MALIAS command is not officially supported in .ALTER blocks.
See Also
.OPTION MEASFILE
HSPICE® Command Reference
X-2005.09
17
2: Commands in HSPICE Netlists
.BIASCHK
.BIASCHK
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>
As an element and model monitor:
.BIASCHK type <region=cutoff | linear | saturation>
+ terminal1=t1 <terminal2=t2> <limit=lim>
+ <noise=ns> <max=max> <min=min>
+ <simulation=op | dc | tr | all> <monitor=v | i | w | l>
+ <name=name1, name2, ...>
+ <mname=modname_1, modname_2, ...>
+ <tstart=time1> <tstop=time2> <autostop>
+ <except=name_1,name_2, ...>
Example 1
This example uses the .BIASCHK statement to monitor an expression:
.biaschk 'v(1)' min = 'v(2)*2' simulation= op
Example 2
This example uses the .BIASCHK statement to monitor an element and model
type:
.biaschk nmos terminal1 = vg terminal2 = vs
simulation = tr name = m1
In this example, terminal1 and terminal2 are the terminals between which
you want to check.
Description
The .BIASCHK statement can monitor the voltage bias, current, device-size,
expression and region during analysis, and reports:
18
■
Element name
■
Time
■
Terminals
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.BIASCHK
■
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 BIASCHK summary in
the *.lis file or a file you define in the .OPTION BIASFILE command option.
You can use this command only for active elements, capacitors, and
subcircuits.
If a model name, referenced in an active element statement, 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 sub-circuit name (123 model
in the x subcircuit).
More than one simulation type or all simulation types can be set in
one .BIASCHK command, and more than one region can be set in
one .BIASCHK command.
Instance (element) and model names can contain wildcards, either “?” (stands
for one character) or “*” (stands for 0 or more characters).
If you do not set name and mname, HSPICE checks all elements of this type for
bias voltage (you must include type in the biaschk card). However, if type =
subckt, at least one name or mname must be specified in the .BIASCHK
command; otherwise, a warning message is issued and this command ignored.
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.
Interactions with Other Options
If you set .OPTION BIAWARN to 1, HSPICE immediately outputs a warning
message that includes the element name, time, terminals and model name
when the limit is exceeded during the analysis you define. If you set the
autostop keyword, HSPICE automatically stops at that situation.
If you set .OPTION BIASFILE, HSPICE outputs the summary into a file you
define in the biasfile. Otherwise, HSPICE outputs the summary to a *.lis file.
HSPICE® Command Reference
X-2005.09
19
2: Commands in HSPICE Netlists
.BIASCHK
Argument
Definition
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, Terminals, between which HSPICE checks (that is, checks between
2
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
Biaschk 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
Biaschk 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
20
Maximum value.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.BIASCHK
Argument
Definition
min
Minimum value.
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:
• 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.
mname
Model 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 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.
• Wildcarding is not supported for mname.
• If only mname is specified in subckt bias check, then all subcircuits
will be checked.
region
Values can be cutoff, linear, or saturation. HSPICE
monitors when the MOS device, defined in the .BIASCHK command,
enters and leaves the specified region (such as cutoff).
simulation The 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.
HSPICE® Command Reference
X-2005.09
21
2: Commands in HSPICE Netlists
.BIASCHK
Argument
Definition
monitor
The kind 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
The biaschk start time during transient analysis. The default is 0.
tstop
The biaschk 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
Lets you specify the element or instance that you do not want to bias
check.
See Also
.OPTION BIASFILE
.OPTION BIAWARN
22
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.CONNECT
.CONNECT
Syntax
.CONNECT node1 node2
Example
...
.subckt eye_diagram node1 node2 ...
.connect node1 node2
...
.ends
This is now 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 statement to node2, apply it to node1 instead. Then, to
change the netlist construction to recognize node2, use a .ALTER statement.
Example 2
*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
The first .TRAN simulation includes two resistors. Later simulations have only
one resistor, because r2 is shorted by connecting cc with 1. v(1) does not
print out, but v(cc) prints out instead.
Use multiple .CONNECT statements to connect several nodes together.
Example 3
.CONNECT node1 node2
.CONNECT node2 node3
HSPICE® Command Reference
X-2005.09
23
2: Commands in HSPICE Netlists
.CONNECT
This example connects both node2 and node3 to node1. All connected nodes
must be in the same subcircuit or all in the main circuit. The first HSPICE
simulation evaluates only node1; node2, and node3 are the same node as
node1. Use .ALTER statements to simulate node2 and node3.
If you set .OPTION NODE, then HSPICE prints out a node connection table.
Description
The .CONNECT statement connects two nodes in your HSPICE netlist so that
simulation evaluates two nodes as only one node. 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.
If you connect node2 to node1, HSPICE does not recognize node2 at all. You
also cannot use this statement in HSPICE RF.
Argument
Definition
node1
Name of the first of two nodes to connect to each other.
node2
Name of the second of two nodes to connect to each other. The first
node replaces this node in the simulation.
See Also
.ALTER
.CONNECT
.OPTION NODE
24
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DATA
.DATA
Syntax
Inline statement:
.DATA datanm pnam1 <pnam2 pnam3 ... pnamxxx >
+
pval1<pval2 pval3 ... pvalxxx>
+
pval1’ <pval2’ pval3’ ... pvalxxx’>
.ENDDATA
External File statement for concatenated data files:
.DATA datanm MER
+ FILE = ’filename1’ pname1 = colnum <pname2 = colnum ...>
+ <FILE = ’filename2’ pname1 = colnum
+ <pname2 = colnum ...>> ... <OUT = ’fileout’>
.ENDDATA
Column Laminated statement:
.DATA datanm LAM
+ FILE = ’filename1’ pname1 = colnum
+ <panme2 = colnum ...>
+ <FILE = ’filename2’ pname1 = colnum
+ <pname2 = colnum ...>> ... <OUT = ’fileout’>
.ENDDATA
Example
* 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
HSPICE or HSPICE RF performs the above analyses for each set of parameter
values defined in the .DATA statement. For example, the program first uses the
width = 50u, length = 30u, thresh = 1.2v, and cap = 1.2pf
parameters to perform .TRAN, .AC, and .DC analyses.
HSPICE or HSPICE RF 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.
HSPICE® Command Reference
X-2005.09
25
2: Commands in HSPICE Netlists
.DATA
Example 2
* .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
This example performs a DC sweep analysis for each set of VBS, VDS, and L
parameters in the .DATA vdot block. That is, HSPICE or HSPICE RF runs
eight DC analyses, one for each line of parameter values in the .DATA block.
Example 3
* .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
In this example:
■
The default start time for the .TRAN analysis is 0.
■
The time increment is 1 ns.
■
The stop time is 100 ns.
This results 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 or HSPICE RF reads the next set of parameter values, and performs
another 100 transient analyses. It sweeps time from 0 to 100 ns in 1 ns steps.
The outer sweep is time, and the inner sweep varies the parameter values.
HSPICE or HSPICE RF performs two hundred analyses: 100 time increments,
times 2 sets of parameter values.
26
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DATA
Example 4
* 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
Example 5
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:
a
a
a
b
b
c
c
a
a
a
b
b
c
c
a
a
a
b
b
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
file is the same as each column of the other files.
The .DATA statement for this example is:
* External File .DATA statement
.DATA inputdata MER
FILE = ‘file1’ p1 = 1 p2 = 3 p3 = 4
FILE = ‘file2’ p1 = 1
FILE = ‘file3’
.ENDDATA
This listing concatenates file1, file2, and file3 to form the inputdata
dataset. The data in file1 is at the top of the file, followed by the data in
file2, and file3. The inputdata in the .DATA statement references the
dataname specified in either the .DC, .AC, or .TRAN analysis statements. The
parameter fields specify the column that contains the parameters (you must
already have defined the parameter names in .PARAM statements). For
HSPICE® Command Reference
X-2005.09
27
2: Commands in HSPICE Netlists
.DATA
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 or HSPICE RF assigns
values of zero to the missing parameters.
Example 6
Three files (D, E, and F) contain the following columns of data:
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. HSPICE RF does not support
column-laminated data files.
The .DATA statement 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
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 statement.
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.
Description
Data-driven analysis syntax requires a .DATA statement, and an analysis
statement that contains a DATA = dataname keyword.
28
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DATA
You can use the .DATA statement 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 statement 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.
The .DATA statement 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 statements can use external and inline data provided in .DATA
statements. 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, no matter how you format the
values.
Each .DATA statement can contain up to 50 parameters. If you need more than
50 parameters in a single .DATA statement, place 50 or fewer parameters in
the .DATA statement, and use .ALTER statements for the remaining
parameters.
HSPICE or HSPICE RF refers to .DATA statements by their datanames so
each dataname must be unique. HSPICE or HSPICE RF support three
.DATA statement formats:
■
Inline data, which is parameter data, listed in a .DATA statement block. The
datanm parameter in a .DC, .AC, or .TRAN analysis statement, calls this
statement. The number of parameters that HSPICE or HSPICE RF 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.
HSPICE® Command Reference
X-2005.09
29
2: Commands in HSPICE Netlists
.DATA
■
Data that is column-laminated from external files. Column lamination means
that the columns of files with the same number of rows, are arranged sideby-side.
To use external files with the .DATA format:
■
Use the MER and LAM keywords to tell HSPICE or HSPICE RF to expect
external file data, rather than inline data.
■
Use the FILE keyword to specify the external filename.
■
You can use simple file names, such as out.dat, without the single or double
quotes ( ‘ ’ or “ ”), but use the quotes when file names start with numbers,
such as “1234.dat”.
■
File names are case sensitive on Unix systems.
For data-driven analysis, specify the start time (time 0) in the analysis
statement so analysis correctly calculates the stop time.
The following shows how different types of analysis use .DATA statements.
Operating point:
.DC 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
30
Argument
Definition
colnum
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 statement.
filenamei
Data file to read. HSPICE or HSPICE RF concatenates files in the order
they appear in the .DATA statement. You can specify up to 10 files.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DATA
Argument
Definition
fileouti
Data file name, where simulation writes concatenated data. This file
contains the full syntax for an inline .DATA statement, and can replace
the .DATA statement 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.
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 statement.
pvali
Parameter value.
See Also
.AC
.DC
.ENDDATA
.PARAM
.TRAN
HSPICE® Command Reference
X-2005.09
31
2: Commands in HSPICE Netlists
.DC
.DC
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>
HSPICE supports the start and stop syntax; HSPICE RF does not.
Data-Driven Sweep:
.DC var1 type np start1 stop1 <SWEEP DATA = datanm>
.DC DATA = datanm<SWEEP var2 start2 stop2 incr2>
.DC DATA = datanm
HSPICE supports the start and stop syntax; HSPICE RF does not.
Monte Carlo:
.DC var1 type np start1 stop1 <SWEEP MONTE = val>
.DC MONTE = val
HSPICE supports Monte Carlo analysis; HSPICE RF does not.
Optimization:
.DC DATA = datanm OPTIMIZE = opt_par_fun
+
RESULTS = measnames MODEL = optmod
.DC var1 start1 stop1 SWEEP OPTIMIZE = OPTxxx
+
RESULTS = measname MODEL = optmod
32
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DC
Example 1
.DC VIN 0.25 5.0 0.25
This example sweeps the value of the VIN voltage source, from 0.25 volts to
5.0 volts in increments of 0.25 volts.
Example 2
.DC VDS 0 10 0.5 VGS 0 5 1
This example 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.
Example 3
.DC TEMP -55 125 10
This example starts a DC analysis of the circuit, from -55°C to 125°C in 10°C
increments.
Example 4
.DC TEMP POI 5 0 30 50 100 125
This script runs a DC analysis, at five temperatures: 0, 30, 50, 100, and 125°C.
Example 5
.DC xval 1k 10k .5k SWEEP TEMP LIN 5 25 125
This example 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.
Example 6
.DC DATA = datanm SWEEP par1 DEC 10 1k 100k
This example specifies a sweep of the par1 value, from 1 k to 100 k in
increments of 10 points per decade.
Example 7
.DC par1 DEC 10 1k 100k SWEEP DATA = datanm
This example also requests a DC analysis, at specified parameters in
the .DATA datanm statement. It also sweeps the par1 parameter, from 1k to
100k in increments of 10 points per decade.
HSPICE® Command Reference
X-2005.09
33
2: Commands in HSPICE Netlists
.DC
Example 8
.DC par1 DEC 10 1k 100k SWEEP MONTE = 30
This example 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
HSPICE supports Monte Carlo analysis; HSPICE RF does not.
Example 9
* Schmitt Trigger Example
*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
.plot v(1) v(5)
.graph dc model = schmittplot input = v(1)
+ output = v(5) 4.0 5.0
.model schmittplot plot xscal = 1 yscal = 1
+ xmin = .5u xmax = 1.2u
.end
Example 10
.DC par1 DEC 10 1k 100k SWEEP MONTE = 10 firstrun = 11
This example invokes a DC sweep of the par1 parameter from 1k to 100k by
10 points per decade and uses 10 randomly generated (Monte Carlo) values
from 11th to 20th trials.
Example 11
.DC par1 DEC 10 1k 100k SWEEP MONTE = list(10 20:30 35:40 50)
This example 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, followed by the 35th to 40th trials, and finally at the 50th trial.
34
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DC
Description
You can use the .DC statement in DC analysis, to:
■
Sweep any parameter value (HSPICE and HSPICE RF).
■
Sweep any source value (HSPICE and HSPICE RF).
■
Sweep temperature range (HSPICE and HSPICE RF).
■
Perform a DC Monte Carlo (random sweep) analysis (HSPICE only; not
supported in HSPICE RF).
■
Perform a data-driven sweep (HSPICE and HSPICE RF).
■
Perform a DC circuit optimization for a data-driven sweep (HSPICE and
HSPICE RF).
■
Perform a DC circuit optimization by using start and stop (HSPICE only; not
supported in HSPICE RF).
■
Perform a DC model characterization (HSPICE only; not supported in
HSPICE RF).
The format for the .DC statement depends on the application that uses it.
Argument
Definition
DATA = datanm
Datanm is the reference name of a .DATA statement.
incr1 …
Voltage, current, element, or model parameters; or temperature
increments.
MODEL
Specifies the optimization reference name. The .MODEL OPT
statement uses this name in an optimization analysis
MONTE = val
val is the number of randomly-generated values, which you can use
to select parameters from a distribution. The distribution can be
Gaussian, Uniform, or Random Limit.
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 statement
RESULTS
Measure name used for optimization in the .MEASURE statement
HSPICE® Command Reference
X-2005.09
35
2: Commands in HSPICE Netlists
.DC
Argument
Definition
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
Indicates that a second sweep has a different type of variation (DEC,
OCT, LIN, POI, or DATA statement; or MONTE = val)
TEMP
Indicates a temperature sweep.
type
Can be any of the following keywords:
•
•
•
•
var1 …
DEC — decade variation
OCT — octave variation
LIN — linear variation
POI — list of points
• 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 statement, and a temperature sweep, then you must
select a parameter name for the source value. A later .DC statement
must refer to this name. The parameter name must not start with V,
I, or TEMP.
In HSPICE RF, you can run a parameter sweep around a single
analysis, but the parameter sweep cannot change any .OPTION
value.
36
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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DC
See Also
.MODEL
.OPTION DCIC
.PARAM
HSPICE® Command Reference
X-2005.09
37
2: Commands in HSPICE Netlists
.DCMATCH
.DCMATCH
Syntax
.DCMATCH OUTVAR <THRESHOLD=T> <FILE=string>
+ <PERTURBATION=P> <INTERVAL=Int>
Example 1
.DCmatch V(9) V(4,2) I(VCC)
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.
Example 2
.DC XVal Start=1K Stop=9K Step=1K
.DCMATCH V(vcc) interval=3
The variable XVal is being sweep 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}.
Description
You use this command to calculate the effects of local variations in device
characteristics on the DC solution of a circuit.
You can perform only one DCMATCH analysis per simulation. Only the last
.DCMATCH statement is used in case more than one in present. The others are
discarded with warnings.
.
Argument
Definition
OUTVAR
Valid node voltages, the difference between node pairs or branch
currents.
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 statements.
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.
38
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DCMATCH
Argument
Definition
FILE
Valid file name for the output tables. Default is basename.dm#
where “#” is the usual sequence number for HSPICE output files.
PERTURBATION Indicates that perturbations of P standard deviation will be used in
calculating the finite difference approximations to device
derivatives. The valid range for P is 0.01 to 6, with a default value
of 2.
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.
See Also
.DC
.MEASURE (Average, RMS, MIN, MAX, INTEG, and PP)
.MEASURE (Equation Evaluation/ Arithmetic Expression)
.MEASURE (FIND and WHEN)
.PROBE
HSPICE® Command Reference
X-2005.09
39
2: Commands in HSPICE Netlists
.DCVOLT
.DCVOLT
Syntax
.DCVOLT V(node1) = val1 V(node2) = val2 ...
.DCVOLT V node1 val1 <node2 val2 ...>
Example
.DCVOLT 11 5 4 -5 2 2.2
Description
Use the .IC statement or the .DCVOLT statement to set transient initial
conditions in HSPICE, but not in HSPICE RF. How it initializes depends on
whether the .TRAN analysis statement includes the UIC parameter.
Note: In HSPICE RF, .IC is always set to OFF.
If you specify the UIC parameter in the .TRAN statement, 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 statement is equivalent to specifying the IC parameter on
each element statement, but is more convenient. You can still specify the IC
parameter, but it does not have precedence over values set in the .IC
statement.
If you do not specify the UIC parameter in the .TRAN statement, HSPICE
computes the DC operating point solution, before the transient analysis. The
node voltages that you specify in the .IC statement are fixed to determine the
DC operating point. HSPICE RF does not output node voltage from operating
point (.OP), if time (t) < 0. Transient analysis releases the initialized nodes
to calculate the second and later time points.
40
Argument
Definition
val1 ...
Specifies voltages. The significance of these voltages depends on
whether you specify the UIC parameter in the .TRAN statement.
node1 ...
Node numbers or names can include full paths or circuit numbers.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DCVOLT
See Also
.IC
.TRAN
HSPICE® Command Reference
X-2005.09
41
2: Commands in HSPICE Netlists
.DEL LIB
.DEL LIB
Syntax
.DEL LIB ‘<filepath>filename’ entryname
.DEL LIB libnumber entryname
Example 1
This example uses an .ALTER block so it applies to HSPICE but not to
HSPICE RF.
FILE1: ALTER1 TEST CMOS INVERTER
.OPTION ACCT LIST
.TEMP 125
.PARAM WVAL = 15U VDD = 5
*
.OP
.DC VIN 0 5 0.1
.PLOT 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
$PROTECTION
.PROT
$protect statements
$below .PROT
.LIB 'MOS.LIB' FAST
$get fast model library
.UNPROT
.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
VDD 1 0 5.5
$using 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
42
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DEL LIB
.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
Example 1 calculates a DC transfer function for a CMOS inverter.
1. First, 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.
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. Use
the .MEASURE statement to measure the rise time of the inverter.
Example 2
This example uses an .ALTER block so it applies to HSPICE but not to
HSPICE RF.
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
.PLOT 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
HSPICE® Command Reference
X-2005.09
43
2: Commands in HSPICE Netlists
.DEL LIB
$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
In this example, 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.
Description
Use the .DEL LIB statement to remove library data from memory. The next
time you run a simulation, the .DEL LIB statement removes the .LIB call
statement with the same library number and entry name, from memory. You
can then use a .LIB statement to replace the deleted library.
You can use the .DEL LIB statement with the .ALTER statement. HSPICE
RF does not support the .ALTER statement.
44
Argument
Definition
entryname
Entry name, used in the library call statement to delete.
filename
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 quote marks.
filepath
Path name of a file, if the operating system supports tree-structured
directories.
libnumber
Library number, used in the library call statement to delete.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DEL LIB
See Also
.ALTER
.LIB
HSPICE® Command Reference
X-2005.09
45
2: Commands in HSPICE Netlists
.DISTO
.DISTO
Syntax
.DISTO Rload <inter <skw2 <refpwr <spwf>>>>
Example
.DISTO RL 2 0.95 1.0E-3 0.75
Description
The .DISTO statement computes the distortion characteristics of the circuit in
an AC small-signal, sinusoidal, steady-state analysis. You can use the .DISTO
statement in HSPICE, but not in HSPICE RF.
The program 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 statement 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. HSPICE RF does
not support the .DISTO statement. If your design contains more than
one .DISTO statement, HSPICE runs only the last statement. The .DISTO
statement 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.
.
46
Argument
Definition
Rload
The resistor element name of the output load resistor, into which the
output power feeds.
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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DISTO
Argument
Definition
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.
spwf
Amplitude of the second frequency (F2). The value must be ≥ 1e-3.
Default = 1.0.
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 or .PLOT
statement.
• 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 statement. 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
statement to limit the amount of output generated.
.DISTO
Value
Description
DIM2
Intermodulation distortion, first difference. Relative magnitude and
phase of the frequency component (F1 - F2).
DIM3
Intermodulation distortion, second difference. The relative
magnitude and phase of the frequency component (2 ⋅ F1 - F2).
HD2
Second-order harmonic distortion. Relative magnitude and phase of
the frequency component 2 ⋅ F1 (ignores F2).
HSPICE® Command Reference
X-2005.09
47
2: Commands in HSPICE Netlists
.DISTO
.DISTO
Value
Description
HD3
Third-order harmonic distortion. Relative magnitude and phase of
the frequency component 3 ⋅ F1 (ignores F2).
SIM2
Intermodulation distortion, sum. Relative magnitude and phase of
the frequency component (F1 + F2).
See Also
.AC
48
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DOUT
.DOUT
Syntax
.DOUT nd VTH ( time state < time state > )
.DOUT nd VLO VHI ( time state < time state > )
The first syntax specifies a single threshold voltage, VTH. A voltage level above
VTH is high; any level below VTH is low.
The second syntax defines a threshold for both a logic high (VHI) and low
(VLO).
Note: If you specify VTH, VLO, and VHI in the same statement, then only VTH
is processed, and VLO and VHI are ignored.
Example
.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)
The .PARAM statement in this example sets the VTH variable value to 3.
The .DOUT statement, 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 1ns, the expected state is logic-high.
■
At 2ns, 3ns, and 4ns, the expected state is “do not care”.
■
At 5ns, the expected state is again logic low.
Description
The digital output (.DOUT) statement specifies the expected final state of an
output signal.
During simulation, HSPICE or HSPICE RF compares simulation results with
the expected output. If the states are different, an error report results.
HSPICE® Command Reference
X-2005.09
49
2: Commands in HSPICE Netlists
.DOUT
Argument
Definition
nd
Node name.
time
Absolute timepoint.
state
Expected condition of the nd node at the specified time:
• 0 expect ZERO,LOW.
• 1 expect ONE,HIGH.
• else Don’t care.
VTH
Single voltage threshold.
VLO
Voltage of the logic-low state.
VHI
Voltage of the logic-high state.
For both syntax cases, the time, state pair describes the expected output.
During simulation, the simulated results are compared against the expected
output vector. If the states are different, HSPICE RF reports an error message.
Legal values for state are:
50
.DOUT
State Value
Description
0
expect ZERO
1
expect ONE
X, x
do not care
U, u
do not care
Z, z
expect HIGH IMPEDANCE (don’t care). HSPICE RF cannot detect
a high impedance state so it treats Z, z as “don’t care” state.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.DOUT
See Also
.GRAPH
.MEASURE
.PARAM
.PLOT
.PRINT
.PROBE
.STIM
HSPICE® Command Reference
X-2005.09
51
2: Commands in HSPICE Netlists
.EBD
.EBD
Syntax
.EBD ebdname
+ file = ’filename’
+ model = ’modelname’
+ component = ’compname:reference_designator’
+ {component = ’compname:reference_designator’...}
Example
.ebd ebd
+ file = ’test.ebd’
+ model = ’16Meg X 8 SIMM Module’
+ component = ’cmpnt:u21’
.ibis cmpnt
+ file = ’ebd.ibs’
+ component = ’SIMM’
+ hsp_ver = 2003.09 nowarn
This example corresponds to the following .ebd file:
...................
[Begin Board Description]
..................
[Pin List] signal_name
J25
POWER5
[Path Description] CAS_2
Pin J25
Len = 0.5 L=8.35n C=3.34p
Node u21.1
Len = 0.5 L=8.35n C=3.34p
Node u22.2
Len = 0.5 L=8.35n C=3.34p
Node u23.3
16Meg X 8 SIMM Module
R=0.01 /
R=0.01 /
R=0.01 /
Description
The .EBD command provides the IBIS(V 3.2) EBD feature. HSPICE uses
the .ebd file when simulating the line connected with the u21
reference_designator. The format of node names is ebdname_SignalName.
For example, the format of a node name called J25 is ebd_POWER5 (see
Figure 1).
52
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.EBD
Argument
Definition
compname
Name of a .ibs file that describes a component.
reference_designator Reference designator that maps the component.
Figure 1
Circuit Connection for EBD Example
J25
Len=0.5
Pin1
U21
Len=0.5
Pin2
U22
Len=0.5
Pin3
U23
See Also
.IBIS
.PKG
HSPICE® Command Reference
X-2005.09
53
2: Commands in HSPICE Netlists
.ELSE
.ELSE
Syntax
.ELSE
Description
.ELSE precedes one or more commands in a conditional block, after the
last .ELSEIF statement, but before the .ENDIF statement. HSPICE executes
these commands by default, if the conditions in the preceding .IF statement,
and in all of the preceding .ELSEIF statements in the same conditional block,
are all false.
For the syntax and a description of how to use the .ELSE statement within the
context of a conditional block, see the .IF statement.
See Also
.ELSEIF
.ENDIF
.IF
54
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.ELSEIF
.ELSEIF
Syntax
.ELSEIF
Description
HSPICE executes the commands that follow the first.ELSEIF statement, only
if condition1 in the preceding .IF statement is false, and condition2 in the
first .ELSEIF statement is true.
If condition1 in the .IF statement and condition2 in the first .ELSEIF
statement are both false, then HSPICE moves on to the next .ELSEIF
statement, if there is one. If this second .ELSEIF condition is true, HSPICE
executes the commands that follow the second .ELSEIF statement, instead of
the commands after the first .ELSEIF statement.
HSPICE ignores the commands in all false .IF and .ELSEIF statements, until
it reaches the first .ELSEIF condition that is true. If no .IF or .ELSEIF
condition is true, HSPICE continues to the .ELSE statement
For the syntax and a description of how to use the .ELSEIF statement within
the context of a conditional block, see the .IF statement.
See Also
.ELSE
.ENDIF
.IF
HSPICE® Command Reference
X-2005.09
55
2: Commands in HSPICE Netlists
.END
.END
Syntax
.END <comment>
Example
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
.PLOT TRAN V(1) (0,5) LX18(M1) LX19(M1) LX20(M1)
+ (0,6E-13)
.END MOS CAPS
Description
An .END statement must be the last statement in the input netlist file. The
period preceding END is a required part of the statement.
Any text that follows the .END statement is a comment, and has no effect on
that simulation.
An input file that contains more than one simulation run must include an .END
statement for each simulation run. You can concatenate several simulations
into a single file.
56
Argument
Definition
<comment>
Can be any comment. Typically, the comment is the name of the netlist
file or of the simulation run, that this command terminates.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.ENDDATA
.ENDDATA
Syntax
.ENDDATA
Description
Use the .ENDDATA statement to end a .DATA block in an HSPICE input netlist.
See Also
.DATA
HSPICE® Command Reference
X-2005.09
57
2: Commands in HSPICE Netlists
.ENDIF
.ENDIF
Syntax
.ENDIF
Description
The .ENDIF statement ends a conditional block of commands that begins with
an .IF statement.
For the syntax and a description of how to use the .ENDIF statement within the
context of a conditional block, see the .IF statement.
See Also
.ELSE
.ELSEIF
.IF
58
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.ENDL
.ENDL
Syntax
.ENDL
Description
Use the .ENDL statement to end a .LIB statement in an HSPICE input netlist.
See Also
.LIB
HSPICE® Command Reference
X-2005.09
59
2: Commands in HSPICE Netlists
.ENDS
.ENDS
Syntax
.ENDS <SUBNAME>
Example 1
.ENDS mos_circuit
This example terminates a subcircuit named mos_circuit.
Example 2
.ENDS
If you omit the subcircuit name as in this second example, this statement
terminates all subcircuit definitions that begin with a .SUBCKT statement.
Description
Use the .ENDS statement to terminate a .SUBCKT statement.
This statement must be the last for any subcircuit definition that starts with
a .SUBCKT command.
You can nest subcircuit references (calls) within subcircuits in HSPICE or
HSPICE RF. However, in HSPICE RF, you cannot replicate output commands
within subcircuit (subckt) definitions.
Argument
Definition
<SUBNAME>
Name of the subcircuit description to terminate, that begins with
a .SUBCKT command.
See Also
.SUBCKT
60
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.EOM
.EOM
Syntax
.EOM <SUBNAME>
Example 1
.EOM diode_circuit
This example terminates a subcircuit named diode_circuit.
Example 2
.EOM
If you omit the subcircuit name as in this second example, this statement
terminates all subcircuit definitions that begin with a .MACRO statement.
Description
Use the .EOM statement to terminate a .MACRO statement.
This statement must be the last for any subcircuit definition that starts with
a .MACRO command.
You can nest subcircuit references (calls) within subcircuits in HSPICE or
HSPICE RF. However, in HSPICE RF, you cannot replicate output commands
within subcircuit (subckt) definitions.
Argument
Definition
<SUBNAME> Name of the subcircuit description to terminate, that begins with
a .SUBCKT command.
See Also
.MACRO
HSPICE® Command Reference
X-2005.09
61
2: Commands in HSPICE Netlists
.FFT
.FFT
Syntax
.FFT <output_var> <START=value> <STOP=value>
+ <NP=value> <FORMAT=keyword>
+ <WINDOW=keyword> <ALFA=value>
+ <FREQ=value> <FMIN=value> <FMAX=value>
Example 1
.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
Example 2
.FFT v(1) np=1024
.FFT v(2) np=1024
This example generates an .ft0 file for the FFT of v(1), and an .ft1 file for the
FFT of v(2).
Description
The .FFT statement uses internal time point values to calculate the Discrete
Fourier Transform (DFT) value, which HSPICE uses for spectrum analysis. A
DFT uses sequences of time values to determine the frequency content of
analog signals in circuit simulation.
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:
.FFT v(1) v(2) np=1024
62
Argument
Definition
output_var
Can be 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 statement, which defaults to 0.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.FFT
Argument
Definition
FROM
An alias for START in .FFT statements.
STOP
End of the output variable waveform to analyze. Defaults to the TSTOP
value in the .TRAN statement.
TO
An alias for STOP, in .FFT statements.
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. Default=1024.
FORMAT
Specifies the output format:
• NORM= normalized magnitude (default)
• UNORM=unnormalized magnitude
WINDOW
Specifies the 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.
Parameter to use in GAUSS and KAISER windows to control the
highest side-lobe level, bandwidth, and so on.
1.0 <= ALFA <= 20.0
Default=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. Default=0.0 (Hz).
HSPICE® Command Reference
X-2005.09
63
2: Commands in HSPICE Netlists
.FFT
Argument
Definition
FMIN
Minimum frequency for which HSPICE prints FFT output into the listing
file. THD calculations also use this frequency.
T = (STOP-START)
Default=1.0/T (Hz).
FMAX
Maximum frequency for which HSPICE prints FFT output into the listing
file. THD calculations also use this frequency. Default=0.5*NP*FM IN
(Hz).
See Also
.TRAN
64
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.FOUR
.FOUR
Syntax
.FOUR freq ov1 <ov2 ov3 ...>
Example
.FOUR 100K V(5)
Description
This statement performs a Fourier analysis as part of the transient analysis.
You can use the .FOUR statement in or HSPICE RF to HSPICE 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 or HSPICE RF 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 or HSPICE RF 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 or HSPICE RF uses 10 frequency bins. The Fourier
analysis determines the DC component, and the first nine AC components. For
improved accuracy, the .FOUR statement can use non-linear, instead of linear
interpolation.
You can only use a .FOUR statement in conjunction with a .TRAN statement.
Argument
Definition
freq
Fundamental frequency
ov1 …
Output variables to analyze.
See Also
.TRAN
HSPICE® Command Reference
X-2005.09
65
2: Commands in HSPICE Netlists
.FSOPTIONS
.FSOPTIONS
Syntax
.FSOPTIONS name <ACCURACY=LOW|MEDIUM|HIGH> +
<GRIDFACTOR=val> <PRINTDATA=YES|NO>
+ <COMPUTEG0=YES|NO> <COMPUTEGD=YES|NO>
+ <COMPUTERO=YES|NO> <COMPUTERS=YES|NO>
Description
Use the .FSOPTIONS statement to set various options for the field solver. The
following rules apply to the Field Solver when specifying options with
the .FSOPTIONS statement:
■
The field solver always computes the L and C matrices.
■
If COMPUTERS=YES, then the field solver starts, and calculates Lo, Ro, and
Rs.
■
For each accuracy mode, the field solver uses either the pre-defined 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 pre-defined 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.
Argument
Definition
name
Option name.
ACCURACY
Sets the solver accuracy to one of the following:
• LOW
• MEDIUM
• HIGH
GRIDFACTOR
Multiplication factor (integer) to determine the final number of
segments used to define the shape.
If you set COMPUTERS=yes, the field solver does not use this
parameter to compute Ro and Rs values.
PRINTDATA
66
The solver prints output matrices.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.FSOPTIONS
Argument
Definition
COMPUTEGO
The solver computes the static conductance matrix.
COMPUTEGD
The solver computes the dielectric loss matrix.
COMPUTERO
The solver computes the DC resistance matrix.
COMPUTERS
The solver computes the skin-effect resistance matrix. This
parameter uses the filament method solver to compute Ro and Rs.
See Also
.LAYERSTACK
.MATERIAL
.SHAPE
HSPICE® Command Reference
X-2005.09
67
2: Commands in HSPICE Netlists
.GLOBAL
.GLOBAL
Syntax
.GLOBAL node1 node2 node3 ...
Example
This example shows global definitions for VDD and input_sig nodes.
.GLOBAL VDD input_sig
Description
The .GLOBAL statement globally assigns a node name in HSPICE or HSPICE
RF. 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 statement is if your netlist file includes
subcircuits. This statement assigns a common node name to subcircuit nodes.
Another common use of .GLOBAL statements is to assign power supply
connections of all subcircuits. For example, .GLOBAL VCC connects all
subcircuits with the internal node name VCC.
Ordinarily, in a subcircuit, the node name consists of the circuit number,
concatenated to the node name. When you use a .GLOBAL statement,
HSPICE or HSPICE RF 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.
68
Argument
Definition
node1 node2
Name of a global nodes, such as supply and clock names; overrides
local subcircuit definitions.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.GRAPH
.GRAPH
Note: This is an obsolete command. You can gain the same functionality by
using the .PROBE command.
Syntax
.GRAPH antype <MODEL = mname> <unam1 = > ov1,
+ <unam2 = >ov2 ... <unamn = >ovn (plo,phi)
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
Description
Use the .GRAPH statement when you need high-resolution plots of HSPICE
simulation results. You cannot use .GRAPH statements in the PC version of
HSPICE or in any versions of HSPICE RF.
Each .GRAPH statement 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 statements (HSPICE only).
Argument
Definition
antype
Type of analysis for the specified plots (outputs). Analysis types are:
DC, AC, TRAN, NOISE, or DISTO (you cannot run DISTO analysis in
HSPICE RF).
mname
Plot model name, referenced in the .GRAPH statement. 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.
HSPICE® Command Reference
X-2005.09
69
2: Commands in HSPICE Netlists
.GRAPH
Argument
Definition
ov1 …
Output variables to print. Can be voltage, current, or element template
variables (HSPICE only; HSPICE RF does not support element
template output, or .GRAPH statements), from a different type of
analysis. You can also use algebraic expressions as output variables,
but you must define them inside the PAR( ) statement.
plo, phi
Lower and upper plot limits. Set the plot limits only at the end of
the .GRAPH statement.
See Also
.DOUT
.MEASURE
.PLOT
.PRINT
.PROBE
.STIM
70
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.HDL
.HDL
Syntax
.HDL filename
Example 1
.hdl "/myhome/Verilog_A_lib/res.va"
This example loads the res.va Verilog-A model file from the /myhome/
Verilog_A_lib directory.
Example 2
.hdl "va_models"
This example loads the va_models.va Verilog-A model file (not va_model file)
from the current working directory.
Description
This .HDL command specifies the Verilog-A source name and path within the
netlist. The Verilog-A file is assumed to have a *.va extension only when a
prefix is provided.
In .MODEL statements, 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 card(s) 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.
HSPICE® Command Reference
X-2005.09
71
2: Commands in HSPICE Netlists
.IBIS
.IBIS
Syntax
.IBIS cname keyword_1 = value_1 ...
+ [keyword_M= value_M]
Example
.ibis cmpnt
+ file = ’ebd.ibs’
+ component = ’SIMM’
+ hsp_ver = 2002.4 nowarn package = 2
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
...................
72
L_pin
C_pin
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.IBIS
Figure 2
Equivalent Circuit for EBD Example
Component cmpnt
buffer cmpnt_nd1
cmpnt_nd1
cmpnt_nd1_i
0.4p
40.0m
2n
gnd
buffer cmpnt_nd2
cmpnt_nd2
cmpnt_nd2_i
0.5p
50.0m
3n
gnd
Description
This is the general syntax for the .IBIS command when used with a
component. The optional keywords are in square brackets.
Argument
Definition
cname
Instance name of this ibis command
HSPICE® Command Reference
X-2005.09
73
2: Commands in HSPICE Netlists
.IBIS
Argument
Definition
keyword_i=
value_i
Assigns the value_i value to the keyword_i keyword. Required
keywords are:
• file=’file_name’ identifies the IBIS file. The file_name parameter
must be lower case and must specify either the absolute path for the
file or the path relative to the directory from which you run the
simulation. For example:
file = ’.ibis/at16245.ibs’
file = ’/home/oneuser/ibis/models/abc.ibs’
• component=’component_name’ identifies the component for
an .ibis command from the IBIS file, specified using the file=’...’
keyword. The component_name keyword is case-sensitive, and it
must match one of the components from the IBIS file. For example:
component = ’procfast’
component = ’Virtex_SSTL_3-I_BG432’
component = ’10_pdref’ $ SPICE-formatted [Pin]
74
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.IBIS
Argument
Definition
keyword_m= Optional keywords:
value_m
• package = [0|1|2|3] (default is 3)
• 0, does not add the rlc package into the component.
• 1, adds [Package] (in .ibs file).
• 2, adds [Pin] (in .ibs file).
• 3, If [Package Model] is defined, set package with package model. If
it is not defined, set package with [Pin]. If the package information is
not set in [Pin], set package with [Package] as a default. Package
Model can be defined in either the IBIS file or the PKG file.
• The following optional keywords are the same as for the B Element
(I/O buffer). For more information, see “Specifying Common
Keywords” in the Modeling Input/Output Buffers Using IBIS chapter
of the HSPICE Signal Integrity Guide.
• typ
• interpo
• ramp_rwf
• ramp_fwf
• rwf_tune
• fwf_tune
• pd_scal
• pu_scal
• pc_scal
• gc_scal
• rwf_scal
• fwf_scal
• nowarn
• hsp_ver
• c_com_pu
• c_com_pd
• c_com_pc
• c_com_gc
See Also
.EBD
.PKG
HSPICE® Command Reference
X-2005.09
75
2: Commands in HSPICE Netlists
.IC
.IC
Syntax
.IC V(node1) = val1 V(node2) = val2 ...
Example
.IC V(11) = 5 V(4) = -5 V(2) = 2.2
Description
Use the .IC statement or the .DCVOLT statement to set transient initial
conditions in HSPICE, but not in HSPICE RF. How it initializes depends on
whether the .TRAN analysis statement includes the UIC parameter.
Note: In HSPICE RF, .IC is always set to OFF.
If you specify the UIC parameter in the .TRAN statement, 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 statement is equivalent to specifying the IC parameter on
each element statement, but is more convenient. You can still specify the IC
parameter, but it does not have precedence over values set in the .IC
statement.
If you do not specify the UIC parameter in the .TRAN statement, HSPICE
computes the DC operating point solution before the transient analysis. The
node voltages that you specify in the .IC statement are fixed to determine the
DC operating point. HSPICE RF does not output node voltage from operating
point (.OP), if time (t) < 0. Transient analysis releases the initialized nodes to
calculate the second and later time points.
76
Argument
Definition
val1 ...
Specifies voltages. The significance of these voltages depends on
whether you specify the UIC parameter in the .TRAN statement.
node1 ...
Node numbers or names can include full paths or circuit numbers.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.IC
See Also
.DCVOLT
.TRAN
.OPTION DCIC
HSPICE® Command Reference
X-2005.09
77
2: Commands in HSPICE Netlists
.ICM
.ICM
Syntax
.ICM icmname
+ file = 'icmfilename'
+ model = 'icmmodelname'
Example 1
.ICM icm1
+ file = 'test1.icm'
+ model = 'FourLineModel1'
Example 2
The following example shows how to reference a pin of ICM model in HSPICE
netlist.
icm1_NodeMap1_pin1, icm1_NodeMap2_pin1,
icm1_NodeMap2_pin2, ...
Description
The .ICM command automatically creates 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:
78
■
If the model is described using [Nodal Path Description]
'icmname'_'nodemapname'_'pinname'
■
If the model is described using [Tree Path Description]
'icmname'_'pinmapname'_'pinname'
Argument
Definition
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].
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.IF
.IF
Syntax
.IF (condition1)
...
<.ELSEIF (condition2)
... >
<.ELSE
... >
.ENDIF
Example
.IF (a==b)
.INCLUDE /myhome/subcircuits/diode_circuit1
...
.ELSEIF (a==c)
.INCLUDE /myhome/subcircuits/diode_circuit2
...
.ELSE
.INCLUDE /myhome/subcircuits/diode_circuit3
...
.ENDIF
Description
HSPICE executes the commands that follow the first.ELSEIF statement, only
if condition1 in the preceding .IF statement is false, and condition2 in the
first .ELSEIF statement is true.
If condition1 in the .IF statement and condition2 in the first .ELSEIF
statement are both false, then HSPICE moves on to the next .ELSEIF
statement, if there is one. If this second .ELSEIF condition is true, HSPICE
executes the commands that follow the second .ELSEIF statement, instead of
the commands after the first .ELSEIF statement.
HSPICE ignores the commands in all false .IF and .ELSEIF statements, until
it reaches the first .ELSEIF condition that is true. If no .IF or .ELSEIF
condition is true, HSPICE continues to the .ELSE statement
.ELSE precedes one or more commands in a conditional block, after the
last .ELSEIF statement, but before the .ENDIF statement. HSPICE executes
these commands by default, if the conditions in the preceding .IF statement,
and in all of the preceding .ELSEIF statements in the same conditional block,
are all false.
HSPICE® Command Reference
X-2005.09
79
2: Commands in HSPICE Netlists
.IF
The .ENDIF statement ends a conditional block of commands that begins with
an .IF statement.
Argument
Definition
condcition1
Condition that must be true, before HSPICE executes the commands
that follow the .IF statement.
condition2
Condition that must be true, before HSPICE executes the commands
that follow the .ELSEIF statement. HSPICE executes the commands
that follow condition2, only if condition1 is false and condition2 is true.
See Also
.ELSE
.ELSEIF
.ENDIF
80
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.INCLUDE
.INCLUDE
Syntax
.INCLUDE ‘<filepath> filename’
Example
.INCLUDE /myhome/subcircuits/diode_circuit
Description
You can include a netlist as a subcircuit in one or more other netlists. To include
another netlist in the current netlist, use the .INCLUDE statement.
Argument
Definition
filepath
Path name of a file for computer operating systems that support treestructured directories.
A .INC file can contain nested .INC calls to itself or to another .INC file.
If you use a relative path in a nested .INC call, the path starts from the
directory of the parent .INC file, not from the work directory. If the path
starts from the work directory, HSPICE can also find the .INC file, but
prints a warning.
filename
Name of a file to include in the data file. The file path, plus the file name,
can be up to 1024 characters long. You can use any valid file name for
the computer’s operating system. You must enclose the file path and
name in single or double quotation marks.
HSPICE® Command Reference
X-2005.09
81
2: Commands in HSPICE Netlists
.LAYERSTACK
.LAYERSTACK
Syntax
.LAYERSTACK sname <BACKGROUND=mname>
+ <LAYER=(mname,thickness) ...>
Description
A layer stack defines a stack of dielectric or metal layers.
You must associate each transmission line system with one, and 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) are located only at the bottom, only at the top,
or both at the top and bottom.
■
Layers are stacked in the y-direction, and 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:
.LAYERSTACK halfSpace PEC 0.1mm
Argument
Definition
sname
Layer stack name.
mname
Material name.
BACKGROUND Background dielectric material name. By default, the Field Solver
assumes AIR for the background.
thickness
82
Layer thickness.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.LAYERSTACK
See Also
.FSOPTIONS
.MATERIAL
.SHAPE
HSPICE® Command Reference
X-2005.09
83
2: Commands in HSPICE Netlists
.LIB
.LIB
Syntax
Use the following syntax for library calls:
.LIB ‘<filepath> filename’ entryname
Use the following syntax to define library files:
.LIB entryname1
. $ ANY VALID SET OF HSPICE STATEMENTS
.ENDL entryname1
.LIB entryname2
.
. $ ANY VALID SET OF HSPICE STATEMENTS
.ENDL entryname2
.LIB entryname3
.
. $ ANY VALID ET OF HSPICE STATEMENTS
.ENDL entryname3
Example 1
* Library call
.LIB 'MODELS' cmos1
Example 2
.LIB MOS7
$ Any valid set of HSPICE commands
.
.
.
.ENDL MOS7
Example 3
The following are an illegal example and a legal example of nested .LIB
statements for the file3 library.
Illegal:
.LIB MOS7
...
.LIB 'file3' MOS7 $ This call is illegal in MOS7 library
...
...
.ENDL
84
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.LIB
Legal:
.LIB MOS7
...
.LIB 'file1' MOS8
.LIB 'file2' MOS9
.LIB CTT $ file2 is already open for the CTT
$ entry point
.ENDL
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
This example is a .LIB call statement 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 analysis. The model is in the
/usr/meta/lib/cmos1_mod.dat include file.
.MODEL NCH
+ DELVTO =
.MODEL PCH
+ DELVTO =
NMOS LEVEL = 2 XL = XL TOX = TOX
DELVTON .....
PMOS LEVEL = 2 XL = XL TOX = TOX
DELVTOP .....
The .model keyword (left side) equates to the skew parameter (right side). A
.model keyword can be the same as a skew parameter.
HSPICE® Command Reference
X-2005.09
85
2: Commands in HSPICE Netlists
.LIB
Description
To create and read from libraries of commonly-used commands, device
models, subcircuit analysis, and statements (library calls) in library files, use
the .LIB call statement. As HSPICE or HSPICE RF encounters each .LIB
call name in the main data file, it reads the corresponding entry from the
designated library file, until it finds an .ENDL statement.
You can also place a .LIB call statement in an .ALTER block.
To build libraries (library file definition), use the .LIB statement in a library file.
For each macro in a library, use a library definition statement (.LIB
entryname) and an .ENDL statement.
The .LIB statement begins the library macro, and the .ENDL statement ends
the library macro. The text after a library file entry name must consist of
HSPICE or HSPICE RF statements.
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
statement 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 statement and the .INCLUDE statement to
access the models and skew parameters. The library contains parameters that
modify .MODEL statements.
86
Argument
Definition
filepath
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 or HSPICE RF, you do not need to specify a directory
path; the netlist runs on any machine. Use the “../” syntax in the filepath
to designate the parent directory of the current directory.
entryname
Entry name for the section of the library file to include. The first
character of an entryname cannot be an integer.
filename
Name of a file to include in the data file. The combination of filepath plus
filename 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 the “../” syntax
in the filename to designate the parent directory of the current directory.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.LIB
See Also
.ALTER
.ENDL
.INCLUDE
HSPICE® Command Reference
X-2005.09
87
2: Commands in HSPICE Netlists
.LIN
.LIN
Syntax
.LIN <sparcalc = [1|0] <modelname = ...>>
+ <filename = ...> <format=[selem|citi|touchstone]>
+ <noisecalc = [1|0] <gdcalc = [1|0]>
+ <mixedmode2port = [dd|dc|ds|cd|cc|cs|sd|sc|ss]>
+ <dataformat = [ri|ma|db]>
Example
.LIN sparcalc=1 modelname=my_custom_model
+ filename=mydesign format=touchstone noisecalc=1
+ gdcalc=1 dataformat=ri
This example extracts linear transfer parameters for a general multi-port
network, performs a 2-port noise analysis, and performs a group-delay analysis
for a model named my_custom_model. The output is in the mydesign output
file, which is in the TOUCHSTONE format. The data format in the
TOUCHSTONE file is real-imaginary.
Description
The .LIN command extracts noise and linear transfer parameters for a general
multi-port network.
When used with P (port) element(s) and .AC commands, .LIN makes
available a broad set of linear port-wise measurements:
■
standard and mixed-mode multi-port S (scattering) parameters
■
standard and mixed-mode multi-port Y/Z parameters
■
standard mode multi-port H parameter
■
standard mode two-port noise parameters
■
standard and mixed-mode group delays
■
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.
88
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.LIN
The .LIN command also supports mixed-mode transfer parameters
calculation and group delay analysis when used together with mixed-mode P
elements.
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.
Argument
Definition
sparcalc
If 1, extract S parameters (default).
modelname
Model name listed in the .MODEL statement in the .sc# model
output file.
filename
Output file name (default=netlist name).
format
Output file format:
• selem is for S element .sc# format, which you can include in the
netlist.
• citi is CITIfile format.
• touchstone is TOUCHSTONE file format.
noisecalc
If 1, extract noise parameters (perform 2-port noise analysis).
Default=0.
gdcalc
If 1, extract group delay (perform group delay analysis). Default=0.
HSPICE® Command Reference
X-2005.09
89
2: Commands in HSPICE Netlists
.LIN
Argument
Definition
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:
• 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
dataformat
The dataformat keyword describe the data format output to the
.sc#/touchstone/citi 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 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 digits in citifiles.
90
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.LOAD
.LOAD
Syntax
.LOAD <FILE = load_file> <RUN = PREVIOUS | CURRENT>
Example 1
.TITLE
.SAVE FILE=design.ic
.LOAD FILE=design.ic0
$load--design.ic0 save--design.ic0
.alter
...
$load--none
save--design.ic1
.alter
...
$load--none
save--design.ic2
.end
This example loads a file name design.ic0, which you previously saved
using a .SAVE command.
Example 2
.TITLE
.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
.TITLE
.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
Description
Use the .LOAD statement to input the contents of a file, that you stored using
the .SAVE statement in HSPICE.
HSPICE® Command Reference
X-2005.09
91
2: Commands in HSPICE Netlists
.LOAD
Note: HSPICE RF does not support the .SAVE and .LOAD (save and restart)
statements.
Files stored with the .SAVE statement 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.
Argument
Definition
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=
Used only outside of .ALTER statements in a netlist that
contains .ALTER statements. The format of file name is <design>.ic.
PREVIOUS
Each .ALTER run uses the saved operating point from the
previous .ALTER run in the same simulation.
CURRENT
Each .ALTER run uses the saved operating point from the
current .ALTER run in the last simulation.
See Also
.ALTER
.SAVE
92
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MACRO
.MACRO
In HSPICE RF, you cannot replicate output commands within subcircuit
(subckt) definitions.
Syntax
.MACRO subnam n1 <n2 n3 …> <parnam = val>
.EOM
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
The preceding example defines two subcircuits: SUB1 and SUB2. These are
resistor divider networks, whose resistance values are parameters (variables).
The X1, X2, and X3 statements call these subcircuits. Because the resistor
values are different in each call, these three calls produce different subcircuits.
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
...
HSPICE® Command Reference
X-2005.09
93
2: Commands in HSPICE Netlists
.MACRO
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
...
This example 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.
Description
You can create a subcircuit description for a commonly-used circuit, and
include one or more references to the subcircuit in your netlist.
To define a subcircuit in your netlist, use the .MACRO statement. Use the .EOM
statement to terminate a .MACRO statement.
Argument
Definition
subnam
Specifies a 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, are strictly local with three exceptions:
• Ground node (zero).
• Nodes assigned using BULK = node in MOSFET or BJT models.
• Nodes assigned using the .GLOBAL statement.
94
parnam
A 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 statement.
SubDefaultsList
<SubParam1>=<Expression>
[<SubParam2>=<Expression>...]
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MACRO
See Also
.ENDS
.EOM
.MACRO
.SUBCKT
HSPICE® Command Reference
X-2005.09
95
2: Commands in HSPICE Netlists
.MALIAS
.MALIAS
Syntax
.MALIAS model_name=alias_name1 <alias_name2 ...>
■
model_name is the model name defined in the .model card.
■
alias_name1... is the alias that an instance (element) of the model
references.
Example
*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
■
zendef is a diode model
■
zen and zend are its aliases.
■
The zendef model points to both the zen and zend aliases.
Description
You can use the .MALIAS statement to assign an alias (another name) to a
diode, BJT, JFET, or MOSFET model that you defined in a .MODEL statement.
You cannot use the .MALIAS statement in HSPICE RF.
.MALIAS differs from .ALIAS in two ways:
96
■
A model can define the alias in an .ALIAS statement, but not the alias in
a .MALIAS statement. The .MALIAS statment 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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MALIAS
You can use .MALIAS to alias to a model name that you defined in a .MODEL
statement or to alias to a subcircuit name that you defined in a .SUBCKT
statement. The syntax for .MALIAS is the same in either usage.
Note: Using .MALIAS in .ALTER blocks is not recommended or supported.
See Also
.ALIAS
HSPICE® Command Reference
X-2005.09
97
2: Commands in HSPICE Netlists
.MATERIAL
.MATERIAL
Note: You cannot use the .MATERIAL statement in HSPICE RF.
Syntax
.MATERIAL mname METAL|DIELECTRIC <ER=val>
+ <UR=val> <CONDUCTIVITY=val> <LOSSTANGENT=val>
Description
The field solver assigns the following default values for metal:
■
CONDUCTIVITY = -1 (perfect conductor)
■
ER = 1
■
UR = 1
PEC is a pre-defined metal name. You cannot redefine its default values.
The field solver assigns the following default values for dielectrics:
■
CONDUCTIVITY = 0 (lossless dielectric)
■
LOSSTANGENT = 0 (lossless dielectric)
■
ER = 1
■
UR = 1
AIR is a pre-defined dielectric name. You cannot redefine its default values.
Because the field solver does not currently support magnetic materials, it
ignores UR values.
Argument
Definition
mname
Material name.
METAL|DIELECTRIC Material type: METAL or DIELECTRIC.
98
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 ).
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MATERIAL
See Also
.LAYERSTACK
HSPICE® Command Reference
X-2005.09
99
2: Commands in HSPICE Netlists
.MEASURE
.MEASURE
Description
Use the .MEASURE statement to modify information and to define the results of
successive HSPICE or HSPICE RF simulations. The .MEASURE statement
prints user-defined electrical specifications of a circuit. Optimization (HSPICE
only) uses .MEASURE statements extensively. 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 (HSPICE only), and to curve-fit
measured data to model parameters.
The .MEASURE statement can use several different formats, depending on the
application. You can use it for either DC sweep, AC, or transient analyses.
See Also
.AC
.DC
.DCMATCH
.DOUT
.GRAPH
.OPTION MEASDGT
.OPTION MEASFAIL
.OPTION MEASFILE
.OPTION MEASSORT
.OPTION MEASOUT
.PLOT
.PRINT
.PROBE
.STIM
.TRAN
100
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Rise, Fall, and Delay Measurements)
.MEASURE (Rise, Fall, and Delay Measurements)
Syntax
.MEASURE <DC | AC | TRAN> result TRIG … TARG …
+ <GOAL = val> <MINVAL = val> <WEIGHT = val>
The input syntax for delay, rise time, and fall time in HSPICE RF is:
.MEASURE <TRAN > varname TRIG_SPEC TARG_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 of
TRIG_SPEC and TARG_SPEC is:
TRIG var VAL = val < TD = td > < CROSS = c | LAST >
+ < RISE = r | LAST > < FALL = f | LAST >
+ <TRIG AT = time>
TARG var VAL = val < TD = td > < CROSS = c | LAST >
+ < RISE = r | LAST > < FALL = f | LAST>
+ <TRIG AT = time>
Example 1
* 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
This example 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. The 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 has elapsed. HSPICE prints results as
tdlay = <value>.
Example 2
.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
HSPICE® Command Reference
X-2005.09
101
2: Commands in HSPICE Netlists
.MEASURE (Rise, Fall, and Delay Measurements)
In the last example, TRIG. AT = 10n starts measuring time at t = 10 ns in the
transient analysis. The TARG parameters end time measurement when V(IN) =
2.5 V, on the third crossing. pwidth is the printed output variable.
If you use the .TRAN analysis statement with a .MEASURE statement, do not
use a non-zero start time in .TRAN statement or the .MEASURE results might
be incorrect.
Example 3
.MEAS TRAN TDEL12 TRIG V(signal1) VAL='VDD/2'
+ RISE=10 TARG V(signal2) VAL='VDD/2' RISE=1 TD=TRIG
This example shows a target that is delayed until the trigger time before the
target counts the edges.
Description
Use the Rise, Fall, and Delay form of the .MEASURE statement to measure
independent-variable (time, frequency, or any parameter or temperature)
differential measurements such as rise time, fall time, slew rate, or any
measurement that requires determining independent variable values. This
format specifies TRIG and TARG substatements. These two statements specify
the beginning and end of a voltage or current amplitude measurement.
Argument
Definition
MEASURE
Specifies measurements. You can abbreviate to MEAS.
result
Name associated with the measured value in the HSPICE or
HSPICE RF output. 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…
102
Identifies the beginning of trigger specifications.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Rise, Fall, and Delay Measurements)
Argument
Definition
TARG …
Identifies the beginning of target specifications.The input syntax
for delay, rise time, and fall time in HSPICE RF is:
.MEASURE < TRAN > varname TRIG_SPEC TARG_SPEC
varname is the user-defined variable name for the measurement,
the time difference between TRIG and TARG events.
<DC | AC | TRAN> Specifies the analysis type of the measurement. If you omit this
parameter, HSPICE or HSPICE RF uses the last analysis mode
that you requested.
GOAL
Specifies the 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.
Default = 1.0e-12.
WEIGHT
Multiplies the calculated error by the weight value. Used only in
ERR calculation for optimization. Default = 1.0.
TRIG/TARG
Parameter
Definition
TRIG
Indicates the beginning of the trigger specification.
trig_val
Value of trig_var, which increments the counter for crossings, rises,
or falls, by one.
trig_var
Specifies the name of the output variable, that determines the logical
beginning of a measurement. If HSPICE or HSPICE RF reaches the
target before the trigger activates, .MEASURE reports a negative
value.
TARG
Indicates the beginning of the target signal specification.
HSPICE® Command Reference
X-2005.09
103
2: Commands in HSPICE Netlists
.MEASURE (Rise, Fall, and Delay Measurements)
104
TRIG/TARG
Parameter
Definition
targ_val
Specifies the value of the targ_var, which increments the counter for
crossings, rises, or falls, by one.
targ_var
Name of the output variable, at which HSPICE or HSPICE RF
determines the propagation delay with respect to the trig_var.
time_delay
Amount of simulation time that must elapse, before HSPICE or
HSPICE RF enables the measurement. Simulation counts the
number of crossings, rises, or falls, only after the time_delay value.
Default trigger delay is zero.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Average, RMS, and Peak Measurements)
.MEASURE (Average, RMS, and Peak Measurements)
Syntax
.MEASURE <TRAN > out_var func var
+ FROM = start TO = end
Example 1
.MEAS TRAN RMSVAL RMS V(OUT) FROM = 0NS TO = 10NS
In this example, the .MEASURE statement calculates the RMS voltage of the
OUT node, from 0ns to 10ns. It then labels the result RMSVAL.
Example 2
.MEAS MAXCUR MAX I(VDD) FROM = 10NS TO = 200NS
In this example, the .MEASURE statement finds the maximum current of the
VDD voltage supply, between 10ns and 200ns in the simulation. The result is
called MAXCUR.
Example 3
.MEAS P2P PP PAR(‘V(OUT)/V(IN)’)
+ FROM = 0NS TO = 200NS
In this example, the .MEASURE statement uses the ratio of V(OUT) and V(IN) to
find the peak-to-peak value in the interval of 0ns to 200ns.
Description
This ..MEASURE statement reports the average, RMS, or peak value of the
specified output variable.
HSPICE® Command Reference
X-2005.09
105
2: Commands in HSPICE Netlists
.MEASURE (Average, RMS, and Peak Measurements)
Argument
Definition
varname
User-defined variable name for the measurement.
func
One of the following keywords:
• AVG: Average area under var, divided by the period
of interest.
• MAX: Maximum value of var over the specified
interval.
• MIN: Minimum value of var over the specified
interval.
• PP: Peak-to-peak: reports the maximum value,
minus the minimum of var over the specified
interval.
• RMS: Root mean squared: calculates the square
root of the area under the var2 curve, divided
by the period of interest.
• INTEG: Integral of var over the specified period.
out_var
106
var
Name of the output variable, which can be either the node voltage or
the branch current of the circuit. You can also use an expression,
consisting of the node voltages or the branch current.
start
Starting time of the measurement period.
end
Ending time of the measurement period.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (FIND and WHEN)
.MEASURE (FIND and WHEN)
Syntax
.MEASURE <DC | AC | TRAN> result
+ WHEN out_var = val <TD = val>
+ < RISE = r | LAST > < FALL = f | LAST >
+ < CROSS = c | LAST >
+ <GOAL = val> <MINVAL = val> <WEIGHT = val>
.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>
.MEASURE <DC | AC | TRAN> 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>
.MEASURE <DC | AC | TRAN> 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>
.MEASURE <DC | AC | TRAN> result FIND out_var1
+ AT = val <GOAL = val> <MINVAL = val>
+ <WEIGHT = val>
.MEASURE DC result FIND <DCMATCH_TOTAL |
+ DCMATCH(InstanceName)> AT = val
Example
* 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
In this example, 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.
HSPICE® Command Reference
X-2005.09
107
2: Commands in HSPICE Netlists
.MEASURE (FIND and WHEN)
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.
Description
The FIND and WHEN functions of the .MEASURE statement specify to measure:
■
Any independent variables (time, frequency, parameter).
■
Any dependent variables (voltage or current, for example).
■
Derivative of a dependent variable, if a specific event occurs.
Argument
Definition
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 the above example, rise=2 specifies to measure 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.
108
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (FIND and WHEN)
Argument
Definition
LAST
HSPICE or HSPICE RF 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 statements.
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.
<DC | AC | TRAN> Analysis type for the measurement. If you omit this parameter,
HSPICE or HSPICE RF assumes the last analysis type that you
requested.
FIND
Selects the FIND function.
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 statement in a
parameter sweep.
LAST
Starts measurement at the last CROSS, FALL, or RISE event.
• For CROSS = LAST, measurement starts the last time the
WHEN condition is true for either a rising or falling signal.
• For FALL = LAST, measurement starts the last time the WHEN
condition is true for a falling signal.
• For RISE = LAST, measurement starts the last time the
WHEN condition is true for a rising signal.
LAST is a reserved word. Do not use it as a parameter name in
these .MEASURE statements.
HSPICE® Command Reference
X-2005.09
109
2: Commands in HSPICE Netlists
.MEASURE (FIND and WHEN)
Argument
Definition
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.
Default = 1.0e-12.
out_var(1,2,3)
These variables establish conditions that start a measurement.
result
Name of a measured value in the HSPICE or HSPICE RF output.
TD
Time at which measurement starts.
WEIGHT
Multiplies the calculated error by the weight value. Used only in
ERR calculation for optimization. Default = 1.0.
WHEN
Selects the WHEN function.
DCMATCH
(InstanceName)
.DCMATCH contribution from InstanceName.
DCMATCH_TOTAL .DCMATCH total output variation.
110
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Equation Evaluation/ Arithmetic Expression)
.MEASURE (Equation Evaluation/ Arithmetic Expression)
Syntax
.MEASURE <DC | TRAN | AC> result PARAM = ’equation’
+ <GOAL = val> <MINVAL = val>
.MEASURE TRAN varname PARAM = “expression”
Example
.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’
The first two measurements, V3MAX and V2MIN, set up the variables for the
third .MEASURE statement.
■
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.
Description
Use the Equation Evaluation form of the .MEASURE statement to evaluate an
equation, that is a function of the results of previous .MEASURE statements.
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 statements.
Expressions used in arithmetic expression must not be a function of node
voltages or branch currents. Expressions used in all other .MEASURE
statements can contain either node voltages or branch currents, but must not
use results from other .MEASURE statements.
HSPICE® Command Reference
X-2005.09
111
2: Commands in HSPICE Netlists
.MEASURE (Average, RMS, MIN, MAX, INTEG, and PP)
.MEASURE (Average, RMS, MIN, MAX, INTEG, and PP)
Syntax
.MEASURE <DC | AC | TRAN> result func out_var
+ <FROM = val> <TO = val> <GOAL = val>
+ <MINVAL = val> <WEIGHT = val>
.MEASURE DC results <MAX>
+ <DCMATCH_TOTAL | DCMATCH(InstanceName)>
Example 1
.MEAS TRAN avgval AVG V(10) FROM = 10ns TO = 55ns
This example calculates the average nodal voltage value for node 10, during
the transient sweep, from the time 10 ns to 55 ns. It prints out the result as
avgval.
Example 2
.MEAS TRAN MAXVAL MAX V(1,2) FROM = 15ns
TO = 100ns
This example finds the maximum voltage difference between nodes 1 and 2 for
the time period from 15 ns to 100 ns.
Example 3
.MEAS TRAN MINVAL MIN V(1,2) FROM = 15ns TO = 100ns
.MEAS TRAN P2PVAL PP I(M1) FROM = 10ns TO = 100ns
Description
Average (AVG), RMS, MIN, MAX, and peak-to-peak (PP) measurement modes
report statistical functions of the output variable, rather than analysis values.
112
■
AVG calculates the area under an output variable, divided by the periods of
interest.
■
RMS divides the square root of the area under the output variable square, by
the period of interest.
■
MIN reports the minimum value of the output function, over the specified
interval.
■
MAX reports the maximum value of the output function, over the specified
interval.
■
PP (peak-to-peak) reports the maximum value, minus the minimum value,
over the specified interval.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Average, RMS, MIN, MAX, INTEG, and PP)
AVG, RMS, and INTEG have no meaning in a DC data sweep so if you use
them, HSPICE or HSPICE RF issues a warning message.
Argument
Definition
<DC|AC|TRAN> Specifies the analysis type for the measurement. If you omit this
parameter, HSPICE or HSPICE RF assumes the last analysis mode
that you requested.
FROM
Specifies the initial value for the func calculation. For transient
analysis, this value is in units of time.
TO
Specifies the end of the func calculation.
GOAL
Specifies the .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 statement in a
parameter sweep.
func
Indicates one of the measure statement types:
• AVG (average): Calculates the area under the out_var, divided by
the periods of interest.
• MAX (maximum): Reports the maximum value of the out_var,
over the specified interval.
• MIN (minimum): Reports the minimum 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.
result
Name of the measured value in the output. The value is a function of
the variable (out_var) and func.
out_var
Name of any output variable whose function (func) the simulation
measures.
WEIGHT
Multiplies the calculated error, by the weight value. Used only in ERR
calculation for optimization. Default = 1.0.
HSPICE® Command Reference
X-2005.09
113
2: Commands in HSPICE Netlists
.MEASURE (Average, RMS, MIN, MAX, INTEG, and PP)
Argument
Definition
DCMATCH
.DCMATCH contribution from InstanceName.
(InstanceName)
DCMATCH_TOT .DCMATCH total output variation.
AL
114
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Integral Function)
.MEASURE (Integral Function)
Syntax
.MEASURE <DC | AC | TRAN> result INTEGRAL out_var
+ <FROM = val> <TO = val> <GOAL = val>
+ <MINVAL = val> <WEIGHT = val>
Example
.MEAS TRAN charge INTEG I(cload) FROM = 10ns
+ TO = 100ns
This example calculates the integral of I(cload), from 10 ns to 100 ns.
Description
The INTEGRAL function reports the integral of an output variable, over a
specified period.
The INTEGRAL function (with func), uses the same syntax as the average
(AVG), RMS, MIN, MAX, and peak-to-peak (PP) measurement mode to defined
the INTEGRAL (INTEG).
HSPICE® Command Reference
X-2005.09
115
2: Commands in HSPICE Netlists
.MEASURE (Derivative Function)
.MEASURE (Derivative Function)
Syntax
.MEASURE <DC | AC | TRAN> result DERIVATIVE out_var
+ AT = val <GOAL = val> <MINVAL = val>
+ <WEIGHT = val>
.MEASURE <DC | AC | TRAN> result DERIVATIVE out_var
+ WHEN var2 = val <RISE = r | LAST>
+ <FALL = f | LAST> <CROSS = c | LAST> <TD = tdval>
+ <GOAL = goalval> <MINVAL = minval>
+ <WEIGHT = weightval>
.MEASURE <DC | AC | TRAN> result DERIVATIVE out_var
+ WHEN var2 = var3 <RISE = r | LAST>
+ <FALL = f | LAST> <CROSS = c | LAST> <TD = tdval>
+ <GOAL = goalval> <MINVAL = minval>
+ <WEIGHT = weightval>
Example 1
.MEAS TRAN slew rate DERIV V(out) AT = 25ns
This example calculates the derivative of V(out), at 25 ns.
Example 2
.MEAS TRAN slew DERIV v(1) WHEN v(1) = ’0.90*vdd’
This example calculates the derivative of v(1) when v(1) is equal to 0.9*vdd.
Example 3
.MEAS AC delay DERIV ’VP(output)/360.0’ AT = 10khz
This example calculates the derivative of VP(output)/360.0 when the frequency
is 10 kHz.
Description
The DERIVATIVE function provides the derivative of:
116
■
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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Derivative Function)
Argument
Definition
AT = val
Value of out_var, at which the derivative is found.
CROSS = c
The numbers indicate which occurrence of a CROSS, FALL, or RISE
event starts a measurement.
RISE = r
FALL = f
• 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.
<DC|AC|TRAN> Specifies the analysis type to measure. If you omit this parameter,
HSPICE or HSPICE RF assumes the last analysis mode that you
requested.
DERIVATIVE
Selects the derivative function. You can abbreviate to DERIV.
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 statement in a parameter
sweep.
LAST
Measures when the last CROSS, FALL, or RISE event occurs.
• 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 statements.
MINVAL
HSPICE® Command Reference
X-2005.09
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.
Default = 1.0e-12.
117
2: Commands in HSPICE Netlists
.MEASURE (Derivative Function)
118
Argument
Definition
out_var
Variable for which HSPICE or HSPICE RF finds the derivative.
result
Name of the measured value in the output.
TD
Identifies the time when measurement starts.
var(2,3)
These variables establish conditions that start a measurement.
WEIGHT
Multiplies the calculated error, between result and GOAL, by the
weight value. Used only in ERR calculation for optimization.
Default = 1.0.
WHEN
Selects the WHEN function.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Error Function)
.MEASURE (Error Function)
Syntax
.MEASURE <DC | AC | TRAN> result
+ ERRfun meas_var calc_var
+ <MINVAL = val> < IGNORE | YMIN = val>
+ <YMAX = val> <WEIGHT = val> <FROM = val>
+ <TO = val>
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 or HSPICE RF 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.
Argument
Definition
<DC|AC|TRAN> Specifies the analysis type for the measurement. If you omit this
parameter, HSPICE or HSPICE RF assumes the last analysis mode
that you requested.
result
Name of the measured result in the output.
ERRfun
ERRfun indicates which error function to use: ERR, ERR1, ERR2, or
ERR3.
meas_var
Name of any output variable or parameter in the data statement. M
denotes the meas_var in the error equation.
calc_var
Name of the simulated output variable or parameter in
the .MEASURE statement to compare with meas_var. C is the
calc_var in the error equation.
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 = 1.0e15.
HSPICE® Command Reference
X-2005.09
119
2: Commands in HSPICE Netlists
.MEASURE (Error Function)
120
Argument
Definition
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.
WEIGHT
Multiplies the calculated error, by the weight value. Used only in ERR
calculation for optimization. Default = 1.0.
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.
TO
End of the ERRfun calculation. Default is last value of the sweep
variable.
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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MEASURE (Pushout Bisection)
.MEASURE (Pushout Bisection)
Syntax
.MEASURE TRAN MeasureName MeasureClause
pushout=time <lower/upper>
-or.MEASURE TRAN MeasureName MeasureClause
pushout_per=percentage <lower/upper>
Example 1
.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
In this example, the parameter to be optimized is Delaytime and the
evaluation goal is setup_prop. The Pushout=1.5 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).
Example 2
.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
In this example, 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%.
Description
Pushout is only employed 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.
HSPICE® Command Reference
X-2005.09
121
2: Commands in HSPICE Netlists
.MEASURE (Pushout Bisection)
Argument
Definition
pushout=time
Specifies the time. An appropriate time must be specified to obtain
the pushout result (an absolute time).
pushout_per=
percentage
Defines a 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
Specifies the 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". Default=lower.
122
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MODEL
.MODEL
Syntax
.MODEL mname type <VERSION = version_number>
+ <pname1 = val1 pname2 = val2 ...>
.MODEL mname OPT <parameter=val ...>
The following is the .MODEL syntax for use with .GRAPH:
.MODEL mname PLOT (pnam1 = val1 pnam2 = val2….)
The following syntax is used for a Monte Carlo analysis:
.MODEL mname ModelType (<LEVEL=val>
+ <keyname1=val1><keyname2=val2>
+ <keyname3=val3><LOT</n></distribution>><value>
+ <DEV</n></distribution>><value>...)
+ <VERSION=version_number>
Example 1
.MODEL MOD1 NPN BF=50 IS=1E-13 VBF=50 AREA=2 PJ=3,
+ N=1.05
Example 2
This example shows a .MODEL statement 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
Description
Use the .MODEL command to include an instance (element) of a pre-defined
HSPICE model in your input netlist.
For each optimization within a data file, specify a .MODEL statement. HSPICE
can then execute more than one optimization per simulation run. The .MODEL
optimization statement defines:
■
Convergence criteria.
■
Number of iterations.
■
Derivative methods.
HSPICE® Command Reference
X-2005.09
123
2: Commands in HSPICE Netlists
.MODEL
Argument
Definition
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 .GRAPH, this is the plot model name, referenced
in .GRAPH statements.
type
Selects a model type. Must be one of the following.
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
PLOT plot model for the .GRAPH statement
PMOS p-channel MOSFET model
PNP pnp BJT model
R resistor model
U lossy transmission line model (lumped)
W lossy transmission line model
SP S parameter
124
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MODEL
Argument
Definition
CENDIF
Selects different derivative methods. Default=1.0e-9.
The following calculates the gradient of the RESULTS functions:
||Transpose(Jacobi(F(X))) * F(X)||, where F(X) is the RESULT function
If the resulting gradient is less than CENDIF, HSPICE uses more
accurate but more time-consuming derivative methods. By default,
HSPICE uses faster but less-accurate derivative methods. To use the
more-accurate methods, set CENDIF to a larger value than GRAD.
If the gradient of the RESULTS function is less than GRAD, optimization
finishes before CENDIF takes effect.
• If the value is too large, the optimizer requires more CPU time.
• If the value is too small, the optimizer might not find as accurate an
answer.
CLOSE
Initial estimate of how close parameter initial value estimates are to the
solution. CLOSE 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. Default=1.0.
• If CLOSE is greater than 100, the steepest descent in the
Levenburg-Marquardt algorithm dominates.
• If CLOSE is less than 1, the Gauss-Newton method dominates.
For more details, see L. Spruiell, “Optimization Error Surfaces,” MetaSoftware Journal, Volume 1, Number 4, December 1994.
CUT
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. Default = 2.0.
DEV
(Monte Carlo) DEV tolerance, which is independent (each device varies
independently).
HSPICE® Command Reference
X-2005.09
125
2: Commands in HSPICE Netlists
.MODEL
Argument
Definition
DIFSIZ
Increment change in a parameter value for gradient calculations (∆x =
DIFSIZ ⋅ max(x, 0.1) ). If you specify delta in a .PARAM statement, then
∆x = delta. Default = 1e-3.
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.
GRAD
Represents possible convergence, if the gradient of the RESULTS
function is less than GRAD. Most applications use values of 1e-6 to 1e5. Too large a value can stop the optimizer before finding the best
solution. Too small a value requires more iterations. Default=1.0e-6.
ITROPT
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. Default=20.
LEVEL
Selects an optimizing algorithm.
• LEVEL=1 specifies the Modified Levenberg-Marquardt method. You
would use this setting with multiple optimization parameters and
goals.
• LEVEL=2 specifies the BISECTION method in HSPICE RF. You
would use this setting with one optimization parameter.
• LEVEL=3 specifies the PASSFAIL method. You would use this
setting with two optimization parameter.
This argument is ignored when METHOD has been specified.
126
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) Specifies which of ten random number generators
numbered 0 through 9 are 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.
keyword
(Monte Carlo) Model parameter keyword.
MAX
Sets the upper limit on CLOSE. Use values > 100. Default=6.0e+5.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.MODEL
Argument
Definition
METHOD
Specifies an optimization method.
• METHOD = LM specifies the Modified Levenberg-Marquardt
method.
• METHOD = BISECTION specifies the Bisection method.
• METHOD = PASSFAIL specifies the Passfail method.
This argument supersedes LEVEL when present.
PARMIN
Allows better control of incremental parameter changes, during error
calculations. Default=0.1. This produces more control over the trade-off
between simulation time and optimization result accuracy. To calculate
parameter increments, HSPICE uses the relationship:
Dpar_val = DIFSIZ ⋅ MAX(par_val, PARMIN)
PLOT
A .GRAPH statement model.
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.
When used with .GRAPH, each .GRAPH statement includes several
model parameters. If you do not specify model parameters, HSPICE
uses the default values of the model parameters, described in the
following table. Pnamn is one of the model parameters of a .GRAPH
statement, and valn is the value of pnamn. Valn can be more than one
parameter.
RELIN
Sets the 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. Default=0.001.
RELOUT
Sets the 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.
Default=0.001.
HSPICE® Command Reference
X-2005.09
127
2: Commands in HSPICE Netlists
.MODEL
Argument
Definition
VERSION
HSPICE or HSPICE RF version number. Allows portability of the BSIM
(LEVEL=13) and BSIM2 (LEVEL = 39) models, between HSPICE
releases. HSPICE release numbers, and the corresponding version
numbers, are:
HSPICE release Version number
9007B 9007.02
9007D 9007.04
92A 92.01
92B 92.02
93A 93.01
93A.02 93.02
95.3 95.3
96.1 96.1
The VERSION parameter is valid only for LEVEL 13 and LEVEL 39
models. Use it with HSPICE Release H93A.02 and higher. If you use
the parameter with any other model, or with a release before H93A.02,
HSPICE issues a warning, but the simulation continues.You can also
use VERSION to denote the BSIM3v3 version number only in model
LEVELs 49 and 53. For LEVELs 49 and 53, the HSPVER parameter
denotes the HSPICE or HSPICE RF release number.
128
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.NET
.NET
Syntax
One-Port Network
.NET input <RIN = val>
.NET input <val>
Two-Port Network
.NET output input <ROUT = val> <RIN = val>
Example
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
Description
You can use the .NET statement or HSPICE RF to compute parameters for:
■
Z impedance matrix.
■
Y admittance matrix.
■
H hybrid matrix
■
S scattering matrix.
You can use the .NET statement only in conjunction with the .AC statement.
HSPICE or HSPICE RF also computes:
■
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 statement.
HSPICE® Command Reference
X-2005.09
129
2: Commands in HSPICE Netlists
.NET
Argument
Definition
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. Default=1 ohm.
See Also
.AC
130
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.NODESET
.NODESET
Syntax
.NODESET V(node1) = val1 <V(node2) = val2 ...>
or
.NODESET node1 val1 <node2 val2>
Example
.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
Description
The .NODESET statement initializes all specified nodal voltages for DC
operating point analysis. Use the .NODESET statement to correct convergence
problems in DC analysis. If you set the node values in the circuit close to the
actual DC operating point solution, you enhance convergence of the simulation.
The HSPICE or HSPICE RF simulator uses the NODESET voltages only in the
first iteration to set an initial guess for DC operating point analysis.
Argument
Definition
node1 ...
Node numbers or names can include full paths or circuit numbers.
val1
Specifies voltages.
See Also
.DC
HSPICE® Command Reference
X-2005.09
131
2: Commands in HSPICE Netlists
.NOISE
.NOISE
Syntax
.NOISE ovv srcnam inter
Example
.NOISE V(5) VIN 10
Description
Use the .NOISE and .AC statements to control the noise analysis of the circuit.
You can use the .NOISE statement only in conjunction with the .AC statement.
Argument
Definition
ovv
Nodal voltage output variable. Defines the node at which HSPICE or
HSPICE RF sums the noise.
srcnam
Name of the independent voltage or current source to use as the noise
input reference
inter
Interval at which HSPICE or HSPICE RF 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 or HSPICE RF prints summary for the first frequency, and
once for each subsequent increment of the inter frequency. The noise
report is sorted according to the contribution of each node to the overall
noise level.
See Also
.AC
132
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.OP
.OP
Syntax
.OP <format> <time> <format> <time>... <interpolation>
Example 1
.OP .5NS CUR 10NS VOL 17.5NS 20NS 25NS
This example calculates:
■
Operating point at .05ns.
■
Currents at 10 ns for the transient analysis.
■
Voltages at 17.5 ns, 20 ns and 25 ns for the transient analysis.
Example 2
.OP
This example calculates a complete DC operating point solution.
Description
When you include an .OP statement in an input file, HSPICE or HSPICE RF
calculates the DC operating point of the circuit. You can also use the .OP
statement to produce an operating point during a transient analysis. You can
include only one .OP statement in a simulation.
If an analysis requires calculating an operating point, you do not need to
specify the .OP statement; HSPICE or HSPICE RF calculates an operating
point. If you use a .OP statement, and if you include the UIC parameter in
a .TRAN analysis statement, then simulation omits the time = 0 operating
point analysis, and issues a warning in the output listing.
HSPICE® Command Reference
X-2005.09
133
2: Commands in HSPICE Netlists
.OP
Argument
Definition
format
Any of the following keywords. Only the first letter is required.
Default = ALL
• ALL: Full operating point, including voltage, currents,
conductances, and capacitances. This parameter outputs voltage/
current for the specified time.
• BRIEF: Produces a one-line summary of each element’s voltage,
current, and power. Current is stated in milliamperes, and power is
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
Place this parameter directly after ALL, VOLTAGE, CURRENT, or
DEBUG. It specifies the time at which HSPICE or HSPICE RF prints
the report. HSPICE RF returns node voltages only if time (t) is 0.
interpolation
Selects the 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 statement
(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 statement. HSPICE ignores any word after this
keyword.
See Also
.TRAN
134
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.OPTION
.OPTION
Syntax
.OPTION opt1 <opt2 opt3 ...>
Argument
Definition
opt1 ...
Specifies 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. Options are described in detail in Chapter 3,
Options in HSPICE Netlists.
Example
.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.
Description
You use the .OPTION command to modify various aspects of a Synopsys
HSPICE or HSPICE RF simulation, including:
■
output types
■
accuracy
■
speed
■
convergence
You can set any number of options in one .OPTION statement, and you can
include any number of .OPTION statements in an input netlist file. Most options
default to 0 (OFF) when you do not assign a value by using either .OPTION
<opt> = <val> or the option with no assignment: .OPTION <opt>.
To reset options, set them to 0 (.OPTION <opt> = 0). To redefine an option,
enter a new .OPTION statement; HSPICE or HSPICE RF uses the last
definition.
You can use the following types of options with this command. For detailed
information on individual options, see Chapter 3, Options in HSPICE Netlists.
HSPICE® Command Reference
X-2005.09
135
2: Commands in HSPICE Netlists
.OPTION
■
General Control Options
■
CPU Options
■
Interface Options
■
Analysis Options
■
Error Options
■
Version Option
■
Model Analysis Options
■
DC Operating Point, DC Sweep, and Pole/Zero Options
■
Transient and AC Small Signal Analysis Options
■
Transient Control Options
■
Input/Output Options
■
AC Control Options
■
Common Model Interface Options
■
Verilog-A Options
For instructions on how to use options that are relevant to a specific simulation
type, see the appropriate DC, transient, and AC analysis chapters in the
HSPICE Simulation and Analysis User Guide.
136
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PARAM
.PARAM
Syntax
Simple parameter assignment:
.PARAM <ParamName>=<RealNumber>
Algebraic parameter assignments:
.PARAM <ParamName>=’<AlgebraicExpression>’
.PARAM <ParamName1>=<ParamName2>
User-defined functions:
.PARAM <ParamName>(<pv1>[<pv2>])=’<Expression>’
Pre-defined analysis functions:
.PARAM <FunctionName> = <Value>
Optimized parameter assignment:
.PARAM parameter=OPTxxx (initial_guess, low_limit,
+ upper_limit)
.PARAM parameter=OPTxxx (initial_guess, low_limit,
+ upper_limit, delta)
.PARAM <paramname>=str(‘string’)
Example 1
* Simple parameter assignment
.PARAM power_cylces=256
Example 2
* Numerical parameter assignment
.PARAM TermValue = 1g
rTerm Bit0 0 TermValue
rTerm Bit1 0 TermValue
...
Example 3
* Parameter assignment using expressions
.PARAM Pi
= ’355/113’
.PARAM Pi2
= ’2*Pi’
.PARAM npRatio
= 2.1
HSPICE® Command Reference
X-2005.09
137
2: Commands in HSPICE Netlists
.PARAM
.PARAM nWidth
.PARAM pWidth
Mp1
... <pModelName>
Mn1
... <nModelName>
...
=
=
W
W
3u
’nWidth * npRatio’
= pWidth
= nWidth
Example 4
* Algebraic parameter
.param x=cos(2)+sin(2)
Example 5
* Algebraic expression as an output variable
.PRINT DC v(3) gain=PAR(‘v(3)/v(2)’)
+ PAR(‘V(4)/V(2)’)
Example 6
* My own 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 7
* Pre-defined analysis function
.PARAM mcVar = Agauss(1.0,0.1)
Example 8
.PARAM vtx=OPT1(.7,.3,1.0) uox=OPT1(650,400,900)
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 statement (not shown).
Example 9
.PARAM fltmod = str('bpfmodel')
s1 n1 n2 n3 n_ref fqmodel=fltmod zo=50 fbase=25e6 fmax=1e9
This example shows how you can define and use string parameters.
138
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PARAM
Description
The .PARAM statement defines parameters. Parameters in HSPICE or HSPICE
RF are names that have associated numeric values.
A parameter definition in HSPICE or HSPICE RF always uses the last value
found in the input netlist (subject to local versus 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 or HSPICE RF
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, .PLOT,
or .PROBE statement, use the PAR keyword or HSPICE RF (except that you
cannot use the .PLOT statement in HSPICE RF).
■
A user-defined function assignment is similar to an algebraic parameter.
HSPICE or HSPICE RF 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 deep.
■
A pre-defined analysis function. HSPICE or HSPICE RF 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, that HSPICE
RF does not support:
•
frequency
•
time
•
Monte Carlo functions
HSPICE® Command Reference
X-2005.09
139
2: Commands in HSPICE Netlists
.PARAM
Argument
Definition
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.
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.
delta
140
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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PAT
.PAT
Syntax
.PAT <PatName>=data <RB=val> <R=repeat>
.PAT <patName>=[component 1 ... component n] <RB=val>
+ <R=repeat>
Example 1
The following example shows the .PAT command used for a b-string:
.PAT a1=b1010 r=1 rb=1
Example 2
The following example shows how an existing patname is used to define a new
patname:
.PAT a1=b1010 r=1 rb=1
.PAT a2=a1
Example 3
This example shows a nested structure:
.PAT a1=[b1010 r=1 rb=2 b1100]
Example 4
This final example shows 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
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 (NS), which are two different types of pattern
sources. In this case, a b-string is a series of 1, 0, m, and z states. The NS is a
combination of a b-string and another NS defined in the .PAT command.
The .PAT command can also be used to define a new patname, which can be
a b-string or NS.
You should avoid using a predefined patname to define another patname,
which creates a circular definition. A circular definition is created when a
patname is defined that depends on another patname, which in turn is defined
HSPICE® Command Reference
X-2005.09
141
2: Commands in HSPICE Netlists
.PAT
by the original patname. HSPICE detects circular definitions and issues an
error report.
Nested structures must use brackets “[ ]”, but HSPICE does not support using
multiple brackets in one statement. If you need to use another nested structure
as a component in an NS, define the NS in a new .PAT command.
142
Argument
Definition
data
String of 1, 0, M, or Z that represents a pattern source. The first letter
must be “B,” which represents 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
which 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
The elements that make up a nested structure. Components can be
b-strings or a patnames defined in other .PAT commands.
RB=val
Specifies the 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 NS or bstring. If
R=-1, the repeating operation continues forever. The R must be an
integer. If it is less than -1, it automatically set to 0.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PKG
.PKG
Syntax
.PKG pkgname
+file= ’pkgfilename’
+model= ’pkgmodelname’
Example 1
.pkg p_test
+ file=’processor_clk_ff.ibs’
+ model=’FCPGA_FF_PKG’
Example 2
The following example shows how pin1 is referenced:
p_test_pin1_dia and p_test_pin1
The element name becomes:
w_p_test_pin1_? ? or r_p_test_pin1_? ? ...
Description
The .PKG command provides the IBIS(V 3.2) Package Model feature. It
supports both sections and matrixes.
The .PKG command automatically creates a series of elements (W or rlc). 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.
Argument
Definition
pkgname
package card name
HSPICE® Command Reference
X-2005.09
143
2: Commands in HSPICE Netlists
.PKG
Argument
Definition
pkgfilename
name of a .pkg or .ibs file that contains package models.
pkgmodelname
working model in the .pkg file
See Also
.EBD
.IBIS
144
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PLOT
.PLOT
Note: This is an obsolete command. You can gain the same functionality by
using the .PRINT command.
Syntax
.PLOT antype ov1 <(plo1,phi1)> <ov2> <(plo2,phi2)> ...>
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 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 2
.PLOT
.PLOT
.PLOT
.PLOT
AC ZIN YOUT(P) S11(DB) S12(M) Z11(R)
DISTO HD2 HD3(R) SIM2
TRAN V(5,3) V(4) (0,5) V(7) (0,10)
DC V(1) V(2) (0,0) V(3) V(4) (0,5)
In the last line above, 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).
Description
The .PLOT statement plots the output values of one or more variables in a
selected HSPICE analysis. Each .PLOT statement 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 statement.
You can include wildcards in .PLOT statements (HSPICE only).
HSPICE® Command Reference
X-2005.09
145
2: Commands in HSPICE Netlists
.PLOT
Argument
Definition
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 statements), 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 statement. If you set the plot limits to (0,0)
HSPICE automatically sets the plot limits.
See Also
.AC
.DOUT
.GRAPH
.MEASURE
.PRINT
.PROBE
.STIM
146
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PRINT
.PRINT
Syntax
.PRINT antype ov1 <ov2 … >
Example 1
* 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
■
If you replace the .PRINT statement with:
.print TRAN v(din) i(mnx)
then all three cases have identical .sw0 and .tr0 files.
■
If you replace the .print statement with:
.print DC v(din) i(mnx)
then the .sw0 and .tr0 files are different.
Example 2
.PRINT TRAN V (4) I(VIN) PAR(`V(OUT)/V(IN)')
This example 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.
Example 3
.PRINT AC VM(4,2) VR(7) VP(8,3) II(R1)
■
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.
HSPICE® Command Reference
X-2005.09
147
2: Commands in HSPICE Netlists
.PRINT
■
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.
Example 4
.PRINT AC ZIN YOUT(P) S11(DB) S12(M) Z11(R)
This example prints:
■
The magnitude of the input impedance.
■
The phase of the output admittance.
■
Several S and Z parameters.
This statement accompanies a network analysis by using the .AC and .NET
analysis statements.
Example 5
.PRINT DC V(2) I(VSRC) V(23,17) I1(R1) I1(M1)
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.
Example 6
.PRINT NOISE INOISE
This example prints the equivalent input noise.
Example 7
.PRINT DISTO HD3 SIM2(DB)
This example prints the magnitude of third-order harmonic distortion, and the
decibel value of the intermodulation distortion sum, through the load resistor
that you specify in the .DISTO statement (HSPICE only; not supported in
HSPICE RF).
Example 8
.PRINT AC INOISE ONOISE VM(OUT) HD3
148
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PRINT
This statement includes NOISE, DISTO, and AC output variables in the
same .PRINT statement in HSPICE. HSPICE RF supports NOISE and AC
analysis, but not DISTO.
Example 9
.PRINT pj1 = par(‘p(rd) +p(rs)‘)
This statement prints the value of pj1 with the specified function.
HSPICE or HSPICE RF ignores .PRINT statement references to nonexistent
netlist part names, and prints those names in a warning.
Example 10
Derivative function:
.PRINT der=deriv('v(NodeX)')
Integrate function:
.PRINT int = integ('v(NodeX)')
The parameter can be a node voltage, or a reasonable expression.
Example 11
.print p1 = 3
.print p2 = par("p1*5")
You can use p1 and p2 as parameters in netlist. The p1 value is 3; the p2 value
is 15.
Description
The .PRINT statement specifies output variables for which HSPICE or
HSPICE RF prints values. You can include wildcards in .PRINT statements.
You can also use the iall keyword in a .PRINT statement to print all branch
currents of all diode, BJT, JFET, or MOSFET elements in your circuit design.
HSPICE® Command Reference
X-2005.09
149
2: Commands in HSPICE Netlists
.PRINT
Argument
Definition
antype
Type of analysis for outputs. Antype is one of the following types: DC,
AC, TRAN, NOISE, or DISTO (you cannot run DISTO analysis in
HSPICE RF).
ov1 …
Output variables to print. These are voltage, current, or element
template (HSPICE only; HSPICE RF does not support element
template output) variables, from a DC, AC, TRAN, NOISE, or DISTO
analysis (you cannot run DISTO analysis in HSPICE RF).
See Also
.AC
.DC
.OPTION ACOUT
.DISTO
.DOUT
.GRAPH
.MEASURE
.NOISE
.PLOT
.PROBE
.STIM
.TRAN
150
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PROBE
.PROBE
Syntax
.PROBE antype ov1 <ov2 ...>
Example 1
.PROBE DC V(4) V(5) V(1) beta = PAR(`I1(Q1)/I2(Q1)')
Example 2
* Derivative function
.PROBE der=deriv('v(NodeX)')
* Integrate function
.PROBE int = integ('v(NodeX)')
Description
The .PROBE statement saves output variables into interface and graph data
files.The parameter can be a node voltage, or a reasonable expression. You
can include wildcards in .PROBE statements.
Argument
Definition
antype
Type of analysis for the specified plots. Analysis types are: DC, AC,
TRAN, NOISE, or DISTO (you cannot run DISTO analysis in HSPICE
RF).
ov1 …
Output variables to plot: voltage, current, or element template (HSPICE
only; HSPICE RF does not support element template output) variables
from a DC, DCMATCH, AC, TRAN, NOISE, or DISTO analysis (you
cannot run DISTO analysis in HSPICE RF). .PROBE can include more
than one output variable.
HSPICE® Command Reference
X-2005.09
151
2: Commands in HSPICE Netlists
.PROBE
See Also
.AC
.DC
.DCMATCH
.DISTO
.DOUT
.GRAPH
.MEASURE
.NOISE
.PLOT
.PRINT
.STIM
.TRAN
152
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PROTECT
.PROTECT
Syntax
.PROTECT
Description
The .PROTECT statement keeps models and cell libraries private. HSPICE RF
does not support the .PROTECT statement.
■
The .PROTECT statement suppresses printing text from the list file, such as
when you use the BRIEF option.
■
The .UNPROTECT command restores normal output functions.
■
Any elements and models located between a .PROTECT and
an .UNPROTECT statement, 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 within the .PROTECT
and .UNPROTECT statements.
See Also
.UNPROTECT
HSPICE® Command Reference
X-2005.09
153
2: Commands in HSPICE Netlists
.PZ
.PZ
Syntax
.PZ output input
.PZ ov srcname
Example
.PZ
.PZ
V(10)
I(RL)
VIN
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.
Description
The .PZ command performs 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 Applications Manual for
complete information about pole/zero analysis.
For a description of pole/zero options, see Chapter 3, Options in HSPICE
Netlists.
.
Argument
Definition
input
Input source. Can be the name of any independent voltage or current
source.
output
Output variables, which can be:
• Any node voltage, V(n).
• Any branch current, I(branch_name).
154
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.PZ
Argument
Definition
ov
Output variable:
• a node voltage V(n), or
• a branch current I(element)
srcnam
Input source:
• an independent voltage or
• a current source name
See Also
.DC
HSPICE® Command Reference
X-2005.09
155
2: Commands in HSPICE Netlists
.SAMPLE
.SAMPLE
Syntax
.SAMPLE FS = freq <TOL = val> <NUMF = val>
+ <MAXFLD = val> <BETA = val>
Description
To acquire data from analog signals, use the .SAMPLE statement with
the .NOISE and .AC statements to analyze data sampling noise in HSPICE or
HSPICE RF. The SAMPLE analysis performs a noise-folding analysis, at the
output node.
.
Argument
Definition
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). Default = 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. Default = 100.
MAXFLD
Maximum number of folding intervals (default = 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.
See Also
.AC
.NOISE
156
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.SAVE
.SAVE
Syntax
.SAVE <TYPE = type_keyword> <FILE = save_file>
+ <LEVEL = level_keyword> <TIME = save_time>
Example
.TEMP -25 0 25
.SAVE TYPE=NODESET FILE=my_design.ic0 LEVEL=ALL
+ TIME=0
This example saves the operating point corresponding to .TEMP -25 to a file
named my_design.ic0.
Description
The .SAVE statement in HSPICE stores the operating point of a circuit in a file
that you specify. HSPICE RF does not support the .SAVE statement. For quick
DC convergence in subsequent simulations, use the .LOAD statement 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 statement. To not save the
operating point, specify .SAVE LEVEL = NONE.
You can save the operating point data as either an .IC or a .NODESET
statement.
A parameter or temperature sweep saves only the first operating point.
.
Argument
Definition
type_keyword
Storage method for saving the operating point. The type can be one
of the following. Default is NODESET.
• .NODESET: Stores the operating point as a .NODESET
statement. Later simulations initialize all node voltages to these
values, if you use the .LOAD statement. If circuit conditions
change incrementally, DC converges within a few iterations.
• .IC: Stores the operating point as a .IC statement. Later
simulations initialize node voltages to these values if the netlist
includes the .LOAD statements.
save_file
Name of the file that stores DC operating point data. The file name
format is <design>.ic#. Default is <design>.ic0.
HSPICE® Command Reference
X-2005.09
157
2: Commands in HSPICE Netlists
.SAVE
Argument
Definition
level_keyword
Circuit level, at which you save the operating point. The level can be
one of the following.
• 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.
• NONE: Does not save the operating point.
save_time
Time during transient analysis when HSPICE saves the operating
point. HSPICE requires a valid transient analysis statement to save
a DC operating point. Default = 0.
See Also
.IC
.LOAD
.NODESET
158
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.SENS
.SENS
Syntax
.SENS ov1 <ov2 ...>
Example
.SENS V(9) V(4,3) V(17) I(VCC)
Description
The .SENS command obtains DC small-signal sensitivities of output variables
for circuit parameters. You can use this command HSPICE, but not in HSPICE
RF.
If the input file includes a .SENS statement, 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).
You can perform only one .SENS analysis per simulation. Only the last .SENS
statement is used in case more than one in present. The others are discarded
with warnings.
The amount of output generated from a .SENS analysis is dependent on the
size of the circuit.
.
Argument
Definition
ov1 ov2 ...
Branch currents, or nodal voltage for DC component-sensitivity
analysis
HSPICE® Command Reference
X-2005.09
159
2: Commands in HSPICE Netlists
.SENS
See Also
.DC
160
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.SHAPE
.SHAPE
Syntax
.SHAPE sname Shape_Descriptor
Description
Use the .SHAPE statement to define a shape. The Field Solver uses the shape
to describe a cross-section of the conductor.
Argument
Definition
sname
Shape name.
Shape_Descriptor One of the following:
•
•
•
•
Rectangle
Circle
Strip
Polygon
See Also
.FSOPTIONS
.LAYERSTACK
.MATERIAL
HSPICE® Command Reference
X-2005.09
161
2: Commands in HSPICE Netlists
.SHAPE (Defining Rectangles)
.SHAPE (Defining Rectangles)
Syntax
.SHAPE RECTANGLE WIDTH=val HEIGHT=val <NW=val>
+ <NH=val>
Description
Use the RECTANGLE option 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
specify only one of these values and let the solver determine the other.
Figure 3
Coordinates of a Rectangle
y
Width
Height
Origin
(0,0)
162
x
Argument
Definition
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.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.SHAPE (Defining Circles)
.SHAPE (Defining Circles)
Syntax
.SHAPE CIRCLE RADIUS=val <N=val>
Description
The CIRCLE option to defines 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
Figure 4
Coordinates of a Circle
y
Origin
Radius
Starting vertex
of the inscribed
polygon
(0,0)
x
Argument
Definition
RADIUS
Radius of the circle.
N
Number of segments to approximate a circle with a specified radius.
HSPICE® Command Reference
X-2005.09
163
2: Commands in HSPICE Netlists
.SHAPE (Defining Polygons)
.SHAPE (Defining Polygons)
Syntax
.SHAPE POLYGON VERTEX=(x1 y1 x2 y2 ...)
+ <N=(n1,n2,...)>
Example 1
The following rectangular polygon uses the default number of segments:
.SHAPE POLYGON VERTEX=(1 10 1 11 5 11 5 10)
Example 2
The following rectangular polygon uses five segments for each edge:
.SHAPE POLYGON VERTEX=(1 10 1 11 5 11 5 10)
+ N=5
Example 3
Rectangular polygon by using the different number of segments for each edge:
.SHAPE POLYGON VERTEX=(1 10 1 11 5 11 5 10)
+ N=(5 3 5 3)
Description
The .SHAPE POLYGON command option defines a polygon in a Field Solver.
The specified coordinates are within the local coordinate with respect to the
origin of a conductor.
Figure 5
Coordinates of a Polygon
y
Origin
(0,0)
164
x
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.SHAPE (Defining Polygons)
Argument
Definition
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).
HSPICE® Command Reference
X-2005.09
165
2: Commands in HSPICE Netlists
.SHAPE (Defining Strip Polygons)
.SHAPE (Defining Strip Polygons)
Syntax
.SHAPE STRIP WIDTH=val <N=val>
Description
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.
Figure 6
Coordinates of a Strip Polygon
y
Width
Origin
(0,0)
166
x
Argument
Definition
WIDTH
Width of the strip (size in the x-direction).
N
Number of segments that define the strip shape with the specified
width.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.STIM
.STIM
Syntax
General
.STIM <tran|ac|dc> PWL|DATA|VEC
+ <filename=output_filename> ...
PWL Source (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
+
[name1=] ovar1
+
[[name2=]ovar2
+
indepvar=[(]t1
[filename=output_filename]
[node1=n+] [node2=n-]
[node1=n+] [node2=n-] ...]
[t2 ...[)]]
Data Card
.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 (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® Command Reference
X-2005.09
167
2: Commands in HSPICE Netlists
.STIM
Description
You can use the .STIM statement to reuse the results (output) of one
simulation as input stimuli in a new simulation.
The .STIM statement specifies:
■
Expected stimulus (PWL Source, DATA CARD, or VEC FILE).
■
Signals to transform.
■
Independent variables.
One .STIM statement produces one corresponding output file.
PWL Source (Transient Analysis Only):
Argument
Definition
tran
Transient simulation.
filename
Output file name. If you do not specify a file, HSPICE uses the input
filename.
namei
PWL Source Name that you specify. The name must start with V (for
a voltage source) or I (for a current source).
ovar1
Output variable that you specify. ovar can be:
• Node voltage.
• Element current.
• Parameter string. If you use a parameter string, you must specify
name1. You cannot use character strings as parameter values in
HSPICE RF.
For example:
v(1), i(r1), v(2,1), par(’v(1)+v(2)’)
168
node1
Positive terminal node name.
node2
Negative terminal node name.
from
Specifies the time to start output of simulation results. For transient
analysis, uses the time units that you specified.
npoints
Number of output time points.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.STIM
Argument
Definition
to
Specifies the time to end output of simulation results. For transient
analysis, uses the time units that you specified. The from value can
be greater than the to value.
indepvar
Specifies dispersed (independent-variable) time points. You must
specify dispersed time points in increasing order.
Data Card:
Argument
Definition
tran | ac | dc
Selects the simulation type: transient, AC, or DC.
filename
Output file name. If you do not specify a file, HSPICE uses the input
filename.
dataname
Name of the data card to generate.
from
Specifies the time to start output of simulation results. For transient
analysis, uses the time units that you specified.
to
Specifies the time to end output of simulation results. For transient
analysis, uses the time units that you specified.
namei
Name of a parameter of the data card to generate.
npoints
Number of output independent-variable points.
indepvar
Specifies dispersed independent-variable points.
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.
HSPICE® Command Reference
X-2005.09
169
2: Commands in HSPICE Netlists
.STIM
Argument
Definition
ovari
Output variable that you specify. ovar can be:
•
•
•
•
Node voltage.
Element current.
Element templates (HSPICE only).
Parameter string. You cannot use character strings as parameter
values in HSPICE RF.
For example:
v(1), i(r1), v(2,1), par(’v(1)+v(2)’), LX1(m1), LX2(m1)
Digital Vector File (Transient Analysis Only):
170
Argument
Definition
namei
Signal name that you specify.
filename
Output file name. If you do not specify a file, HSPICE uses the input
filename.
ovari
Output variable that you specify. ovar can only be a node voltage.
from
Specifies the time to start output of simulation results. For transient
analysis, uses the time units that you specified.
to
Time to the end output of simulation results. For transient analysis,
uses the specified time units.The from value can be greater than the
to value.
npoints
Number of output time points.
indepvar
Specifies dispersed independent-variable points. You must specify
dispersed time points in increasing order.
vth
High voltage threshold.
vtl
Low voltage threshold.
voh
Logic-high voltage for each output signal.
vol
Logic-low voltage for each output signal.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.STIM
See Also
.DOUT
.GRAPH
.MEASURE
.PLOT
.PRINT
.PROBE
HSPICE® Command Reference
X-2005.09
171
2: Commands in HSPICE Netlists
.SUBCKT
.SUBCKT
In HSPICE RF, you cannot replicate output commands within subcircuit
(subckt) definitions.
Syntax
.SUBCKT subnam n1 <n2 n3 …> <parnam = val>
.ENDS
.SUBCKT <SubName><PinList>[<SubDefaultsList>]
.ENDS
.SUBCKT subnam n1 <n2 n3 …> <param=str('string')>
.ENDS
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
The preceding example defines two subcircuits: SUB1 and SUB2. These are
resistor-divider networks, whose resistance values are parameters (variables).
The X1, X2, and X3 statements call these subcircuits. Because the resistor
values are different in each call, these three calls produce different subcircuits.
172
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.SUBCKT
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
...
This example 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 3
* 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
This example implements an IBIS model that uses string parameters to specify
the IBIS file name and IBIS model name.
Description
You can create a subcircuit description for a commonly-used circuit, and
include one or more references to the subcircuit in your netlist.
To define a subcircuit in your netlist, use the .SUBCKT statement.
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.
HSPICE® Command Reference
X-2005.09
173
2: Commands in HSPICE Netlists
.SUBCKT
Use the .ENDS statement to terminate a .SUBCKT statement.
Argument
Definition
subnam
Specifies a 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, are strictly local with three exceptions:
• Ground node (zero).
• Nodes assigned using BULK = node in MOSFET or BJT models.
• Nodes assigned using the .GLOBAL statement.
parnam
A 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 statement.
SubDefaultsList
<SubParam1>=<Expression>
[<SubParam2>=<Expression>...]
See Also
.ENDS
.EOM
.MACRO
.MODEL.MODEL
.OPTION LIST
.PARAM
174
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.TEMP
.TEMP
Syntax
.TEMP t1 <t2 <t3 ...>>
Example 1
.TEMP -55.0 25.0 125.0
The .TEMP statement sets the circuit temperatures for the entire circuit
simulation. To simulate the circuit by using individual elements or model
temperatures, HSPICE or HSPICE RF uses:
■
Temperature as set in the .TEMP statement.
■
.OPTION TNOM setting (or the TREF model parameter).
■
DTEMP element temperature.
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 this example:
■
The .TEMP statement 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°C.
■
HSPICE or HSPICE RF simulates the D2 diode at 100°C.
■
R1 simulates at 70°C.
HSPICE® Command Reference
X-2005.09
175
2: Commands in HSPICE Netlists
.TEMP
Because the diode model statement specifies TREF at 60°C, HSPICE or
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.
Description
To specify the circuit temperature for an HSPICE or HSPICE RF simulation,
use the .TEMP statement, or the TEMP parameter in the .DC, .AC, and .TRAN
statements. HSPICE compares the circuit simulation temperature against the
reference temperature in the .OPTION TNOM control. HSPICE or HSPICE RF
uses the difference between the circuit simulation temperature and the TNOM
reference temperature to define derating factors for component values.
In HSPICE RF, you can use multiple .TEMP statements to specify multiple
temperatures for different portions of the circuit. HSPICE permits only one
temperature for the entire circuit. Multiple definitions of the .TEMP statements
in a circuit behave as a sweep function.
Note: HSPICE allows multiple .TEMP statements in the netlist, and performs
multiple DC, AC or TRAN analyses for each temperature. Do not set the
temperature to the same value multiple times.
Argument
Definition
t1 t2
Temperatures in ×C, at which HSPICE or HSPICE RF simulates the
circuit.
See Also
.AC
.DC
.TEMP
.OPTION TNOM
.TRAN
176
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.TF
.TF
Syntax
.TF ov srcnam
Example
.TF V(5,3) VIN
.TF I(VLOAD) VIN
For the first example, HSPICE or HSPICE RF 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 statement in a single simulation, HSPICE or HSPICE RF runs only the
last .TF statement.
Description
The transfer function statement (.TF) calculates DC small-signal values for
transfer functions (ratio of output variable to input source). You do not need to
specify .OP.
The .TF statement defines small-signal output and input for DC small-signal
analysis. When you use the .TF statement, HSPICE or HSPICE RF computes:
■
DC small-signal value of the transfer function (output/input),.
■
Input resistance.
■
Output resistance.
.
Argument
Definition
ov
Small-signal output variable.
srcnam
Small-signal input source.
See Also
.DC
HSPICE® Command Reference
X-2005.09
177
2: Commands in HSPICE Netlists
.TITLE
.TITLE
Syntax
.TITLE <string_of_up_to_72_characters>
or
<string_of_up_to_72_characters>
Example
.TITLE my-design_netlist
Description
You set the simulation title in the first line of the input file. HSPICE or HSPICE
RF always reads this line, and uses it 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 statement on the first line of the netlist.
However, HSPICE or HSPICE RF does not require the .TITLE syntax.
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 statement appears as
the first line in a file, simulation interprets it as a title, and does not execute it.
An .ALTER statement does not support using the .TITLE statement. To
change a title for a .ALTER statement, place the title content in the .ALTER
statement itself.
178
Argument
Definition
string
Any character string up to 72 characters long.
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.TRAN
.TRAN
Syntax
Single-Point Analysis
.TRAN tincr1 tstop1 <tincr2 tstop2 ...tincrN tstopN>
+ <START = val> <UIC>
Double-Point Analysis
.TRAN tincr1 tstop1 <tincr2 tstop2 ...tincrN tstopN>
+ <START = val> <UIC>
+ <SWEEP var type np pstart pstop>
.TRAN tincr1 tstop1 <tincr2 tstop2 ...tincrN tstopN>
+ <START = val> <UIC>
+ <SWEEP var START="param_expr1"
+ STOP="param_expr2"
+ STEP="param_expr3">
.TRAN tincr1 tstop1 <tincr2 tstop2 ... tincrN tstopN>
+ <START=val> <UIC>
+ <SWEEP var start_expr stop_expr step_expr>
In HSPICE RF, you can run a parameter sweep around a single analysis, but
the parameter sweep cannot change any .OPTION value.
Data-Driven Sweep
.TRAN DATA = datanm (HSPICE only; HSPICE RF does not support
the .TRAN DATA statement)
.TRAN tincr1 tstop1 <tincr2 tstop2 ...tincrN tstopN>
+ <START = val> <UIC> <SWEEP DATA = datanm>
.TRAN DATA = datanm<SWEEP var type np pstart pstop>(HSPICE
only; HSPICE RF does not support the .TRAN DATA statement)
.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>
HSPICE® Command Reference
X-2005.09
179
2: Commands in HSPICE Netlists
.TRAN
HSPICE RF supports the data-driven syntax only for parameter sweeps:
.tran AB sweepdata=name
Monte Carlo Analysis
.TRAN tincr1 tstop1 <tincr2 tstop2 ...tincrN tstopN>
+ <START = val> <UIC> <SWEEP MONTE = list<(>
+ <num1:num2> <num3> <num5:num6> <num7> <)> >
Optimization
.TRAN DATA = datanm OPTIMIZE = opt_par_fun
+ RESULTS = measnames MODEL = optmod
.TRAN <DATA=filename> SWEEP OPTIMIZE=OPTxxx
+ RESULTS=ierr1 ... ierrn MODEL=optmod
Example 1
.TRAN 1NS 100NS
This example performs and prints the transient analysis, every 1 ns for 100 ns.
Example 2
.TRAN .1NS 25NS 1NS 40NS START = 10NS
This example 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.
Example 3
.TRAN 10NS 1US UIC
This example 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 statement (or by IC parameters in element statements) to
calculate the initial conditions.
Example 4
.TRAN 10NS 1US UIC SWEEP TEMP -55 75 10
This example increases the temperature by 10 °C, through the range -55 °C to
75 °C. It also performs transient analysis for each temperature.
Example 5
.TRAN 10NS 1US SWEEP load POI 3 1pf 5pf 10pf
180
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.TRAN
This example analyzes each load parameter value, at 1 pF, 5 pF, and 10 pF.
Example 6
.TRAN data = dataname
This example is a data-driven time sweep. It uses a data file as the sweep
input. If the parameters in the data statement are controlling sources, then a
piecewise linear specification must reference them.
Example 7
.TRAN 10NS 1US SWEEP MONTE = 10 firstrun = 11
This example performs the calculation every 10ns for 1us, from the 11th to
20th Monte Carlo trials.
Example 8
.TRAN 10NS 1US SWEEP MONTE = list(10 20:30 35:40 50)
This example 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.
Description
.TRAN starts a transient analysis, which simulates a circuit at a specific time.
Argument
Definition
DATA = datanm
Data name, referenced in the .TRAN statement (HSPICE only; not
supported in HSPICE RF).
MONTE = val
Produces a specified number (val) of randomly-generated values.
HSPICE uses them to select parameters from a Gaussian, Uniform,
or Random Limit distribution (HSPICE only; not supported in
HSPICE RF).
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.
HSPICE® Command Reference
X-2005.09
181
2: Commands in HSPICE Netlists
.TRAN
Argument
Definition
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 voltage, current, or temperature; or element or model
parameter value.
START
Time when printing or plotting begins. The START keyword is
optional: you can specify a start time without the keyword.
If you use .TRAN with .MEASURE, a non-zero START time can
cause incorrect .MEASURE results. Do not use non-zero START
times in .TRAN statements when you also use .MEASURE.
SWEEP
Indicates that .TRAN specifies a second sweep.
tincr1…
Specifies the printing or plotting increment for printer output, and the
suggested computing increment for post-processing.
tstop1…
Time when a transient analysis stops incrementing by the first
specified time increment (tincr1). If another tincr-tstop pair follows,
analysis continues with a new increment.
UIC
Uses the nodal voltages specified in the .IC statement (or in the IC =
parameters of the various element statements) to calculate initial
transient conditions, rather than solving for the quiescent operating
point.
type
Specifies any of the following keywords:
• 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.
182
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.TRAN
Argument
Definition
var
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 statement, and a temperature sweep, you must choose a
parameter name for the source value, and subsequently refer to it in
the .TRAN statement. The parameter name must not 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
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.
HSPICE® Command Reference
X-2005.09
183
2: Commands in HSPICE Netlists
.UNPROTECT
.UNPROTECT
Syntax
.UNPROTECT
Description
In HSPICE, the .UNPROTECT statement restores normal output functions that
a .PROTECT statement restricted. HSPICE RF does not support
the .UNPROTECT statement.
■
Any elements and models located between .PROTECT and .UNPROTECT
statements, 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 statements.
See Also
.PROTECT
184
HSPICE® Command Reference
X-2005.09
2: Commands in HSPICE Netlists
.VEC
.VEC
Syntax
.VEC ‘digital_vector_file’
Description
You can call a digital vector file from an HSPICE netlist. A digital vector file
consists of three parts:
■
Vector Pattern Definition section
■
Waveform Characteristics section
■
Tabular Data section.
The .VEC file must be a text file. If you transfer it between Unix and Windows,
use text mode.
HSPICE® Command Reference
X-2005.09
185
2: Commands in HSPICE Netlists
.WIDTH
.WIDTH
Syntax
.WIDTH OUT = {80 |132}
Example
.WIDTH OUT = 132 $ SPICE compatible style
.OPTION CO = 132 $ preferred style
Description
Use the .WIDTH statement to define the print-out width in HSPICE.
Permissible values for OUT are 80 and 132. You can also use .OPTION CO to
set the OUT value.
186
Argument
Definition
OUT
Output print width.
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
3
Options in HSPICE Netlists
3
Describes the simulation options you can set using various forms of
the .OPTION command.
You can set a wide variety of HSPICE simulation options using the .OPTION
command. This chapter provides a list of the various options, arranged by task,
followed by detailed descriptions of the individual options.
Options in this chapter fall into the following categories:
■
General Control Options
■
CPU Options
■
Interface Options
■
Analysis Options
■
Error Options
■
Version Option
■
Model Analysis Options
■
DC Operating Point, DC Sweep, and Pole/Zero Options
■
Transient and AC Small Signal Analysis Options
■
Transient Control Options
■
Input/Output Options
HSPICE® Command Reference
X-2005.09
187
3: Options in HSPICE Netlists
General Control Options
■
AC Control Options
■
Common Model Interface Options
■
Verilog-A Options
General Control Options
.OPTION ACCT
.OPTION INGOLD
.OPTION NXX
.OPTION ACOUT
.OPTION LENNAM
.OPTION OPTLST
.OPTION ALT999 or
ALT9999
.OPTION LIST
.OPTION OPTS
OPTION ALTCC
.OPTION MEASDGT
.OPTION PATHNUM
.OPTION ALTCHK
.OPTION NODE
.OPTION PLIM
.OPTION BEEP
.OPTION NOELCK
.OPTION
POST_VERSION
.OPTION BINPRINT
.OPTION NOMOD
.OPTION SEARCH
.OPTION BRIEF
.OPTION NOPAGE
.OPTION STATFL
.OPTION CO
.OPTION NOTOP
.OPTION VERIFY
.OPTION EPSMIN
.OPTION EXPMAX
.OPTION ARTIST
.OPTION MENTOR
.OPTION PROBE
.OPTION CDS
.OPTION MONTECON
.OPTION PSF
.OPTION CSDF
.OPTION POST
.OPTION SDA
.OPTION DLENCSDF
.OPTION POSTLVL
.OPTION ZUKEN
.OPTION MEASOUT
.OPTION POSTTOP
CPU Options
.OPTION CPTIME
.OPTION LIMTIM
Interface Options
188
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
Analysis Options
Analysis Options
.OPTION ASPEC
.OPTION
NOISEMINFREQ
.OPTION SEED
.OPTION FFTOUT
.OPTION PARHIER
.OPTION SPICE
.OPTION DIAGNOSTIC
.OPTION NOWARN
.OPTION LIMPTS
Error Options
.OPTION BADCHR
.OPTION WARNLIMIT
Version Option
.OPTION H9007
Model Analysis Options
General Model Analysis Options
.OPTION DCAP
.OPTION HIER_SCALE
.OPTION TNOM
.OPTION MODSRH
.OPTION MODMONTE
.OPTION XDTEMP
.OPTION SCALE
MOSFET Model Analysis Options
.OPTION CVTOL
.OPTION DEFNRD
.OPTION DEFW
.OPTION DEFAD
.OPTION DEFNRS
.OPTION SCALM
.OPTION DEFAS
.OPTION DEFPD
.OPTION WL
.OPTION DEFL
.OPTION DEFPS
.OPTION WNFLAG
HSPICE® Command Reference
X-2005.09
189
3: Options in HSPICE Netlists
DC Operating Point, DC Sweep, and Pole/Zero Options
Inductor Model Analysis Options
.OPTION GENK
.OPTION KLIM
BJT and Diode Model Analysis Options
.OPTION EXPLI
DC Operating Point, DC Sweep, and Pole/Zero Options
DC Accuracy Options
.OPTION ABSH
.OPTION DI
.OPTION RELMOS
.OPTION ABSI
.OPTION KCLTEST
.OPTION RELV
.OPTION ABSMOS
.OPTION MAXAMP
.OPTION RELVDC
.OPTION ABSTOL
.OPTION RELH
.OPTION ABSVDC
.OPTION RELI
DC Matrix Options
.OPTION ITL1
.OPTION PIVOT
.OPTION PIVTOL
.OPTION ITL2
.OPTION PIVREF
.OPTION SPARSE
.OPTION NOPIV
.OPTION PIVREL
DC Pole/Zero I/O Options
.OPTION CAPTAB
.OPTION DCCAP
.OPTION OPFILE
.OPTION VFLOOR
190
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
Transient and AC Small Signal Analysis Options
DC Convergence Options
.OPTION CONVERGE
.OPTION DV
.OPTION ITLPTRAN
.OPTION CSHDC
.OPTION GMAX
.OPTION NEWTOL
.OPTION DCFOR
.OPTION GMINDC
.OPTION OFF
.OPTION DCHOLD
.OPTION GRAMP
.OPTION RESMIN
.OPTION DCSTEP
.OPTION GSHDC
.OPTION SYMB
.OPTION DCON
.OPTION GSHUNT
.OPTION DCTRAN
.OPTION ICSWEEP
DC Initialization Control Options
.OPTION ABSTOL
.OPTION GDCPATH
.OPTION MAXAMP
.OPTION CAPTAB
.OPTION GRAMP
.OPTION NEWTOL
.OPTION CSHDC
.OPTION GSHDC
.OPTION NOPIV
.OPTION DCCAP
.OPTION GSHUNT
.OPTION OFF
.OPTION DCFOR
.OPTION ICSWEEP
.OPTION PIVOT
.OPTION DCHOLD
.OPTION ITLPTRAN
.OPTION PIVREF
.OPTION DCIC
.OPTION ITL1
.OPTION PIVTOL
.OPTION DCSTEP
.OPTION ITL2
.OPTION RESMIN
.OPTION DV
.OPTION KCLTEST
.OPTION SPARSE
Transient and AC Small Signal Analysis Options
Transient/AC Accuracy Options
.OPTION ABSH
.OPTION DI
.OPTION RELQ
.OPTION ABSV
.OPTION GMIN
.OPTION RELTOL
.OPTION ACCURATE
.OPTION GSHUNT
.OPTION RELV
HSPICE® Command Reference
X-2005.09
191
3: Options in HSPICE Netlists
Transient and AC Small Signal Analysis Options
.OPTION ACOUT
.OPTION MAXAMP
.OPTION RISETIME
.OPTION CHGTOL
.OPTION RELH
.OPTION TRTOL
.OPTION CSHUNT
.OPTION RELI
.OPTION VNTOL
Transient/AC Speed Options
.OPTION AUTOSTOP
.OPTION BYTOL
.OPTION MBYPASS
.OPTION BKPSIZ
.OPTION FAST
.OPTION SCALE
.OPTION BYPASS
.OPTION ITLPZ
Transient/AC Timestep Options
.OPTION ABSVAR
.OPTION FT
.OPTION ITL4
.OPTION DELMAX
.OPTION IMAX
.OPTION ITL5
.OPTION DVDT
.OPTION IMIN
.OPTION TIMERES
.OPTION FS
.OPTION ITL3
Transient/AC Algorithm Options
.OPTION DVTR
.OPTION ITL5
.OPTION PURETP
.OPTION IMAX
.OPTION LVLTIM
.OPTION RUNLVL
.OPTION IMIN
.OPTION MAXORD
.OPTION TRCON
.OPTION ITL3
.OPTION METHOD
.OPTION ITL4
.OPTION MU
.BIASCHK Options
.OPTION BIASFILE
192
.OPTION BIAWARN
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
Transient Control Options
Transient Control Options
Transient Control Method Options
.OPTION BYPASS
.OPTION INTERP
.OPTION TRCON
.OPTION CSHUNT
.OPTION ITRPRT
.OPTION WACC
.OPTION DVDT
.OPTION MAXORD
.OPTION GSHUNT
.OPTION METHOD
Transient Control Tolerance Options
.OPTION ABSH
.OPTION FAST
.OPTION RELTOL
.OPTION ABSV
.OPTION MAXAMP
.OPTION RELV
.OPTION ABSVAR
.OPTION MBYPASS
.OPTION RELVAR
.OPTION ACCURATE
.OPTION MU
.OPTION SLOPETOL
.OPTION BYTOL
.OPTION RELH
.OPTION TIMERES
.OPTION CHGTOL
.OPTION RELI
.OPTION TRTOL
.OPTION DI
.OPTION RELQ
.OPTION VNTOL
Transient Control Limit Options
.OPTION AUTOSTOP
.OPTION FT
.OPTION ITL4
.OPTION BKPSIZ
.OPTION GMIN
.OPTION ITL5
.OPTION DELMAX
.OPTION IMAX
.OPTION RMAX
.OPTION DVTR
.OPTION IMIN
.OPTION RMIN
.OPTION FS
.OPTION ITL3
.OPTION VFLOOR
HSPICE® Command Reference
X-2005.09
193
3: Options in HSPICE Netlists
Input/Output Options
Transient Control Matrix Options
.OPTION GMIN
.OPTION PIVOT
Iteration Count Dynamic Timestep Options
.OPTION IMAX
.OPTION IMIN
Input/Output Options
.OPTION INTERP
.OPTION MEASFILE
.OPTION OPTLST
.OPTION ITRPRT
.OPTION MEASOUT
.OPTION PUTMEAS
.OPTION MEASDGT
.OPTION MEASSORT
.OPTION UNWRAP
.OPTION MEASFAIL
.OPTION MCBRIEF
AC Control Options
.OPTION ABSH
.OPTION DI
.OPTION RELH
.OPTION ACOUT
.OPTION MAXAMP
.OPTION UNWRAP
Common Model Interface Options
.OPTION CMIFLAG
.OPTION CUSTCMI
Verilog-A Options
.OPTION SPMODEL
194
.OPTION VAMODEL
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ABSH
.OPTION ABSH
Syntax
.OPTION ABSH=x
Description
Sets 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. The default is 0.0.
See Also
.OPTION DI
.OPTION RELH
HSPICE® Command Reference
X-2005.09
195
3: Options in HSPICE Netlists
.OPTION ABSI
.OPTION ABSI
Syntax
.OPTION ABSI=x
Description
Sets 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.
The default is 1e-9 when KCLTEST = 0 or 1e-6 for KCLTEST = 1.
See Also
.DC
.OPTION KCLTEST
.TRAN
196
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ABSMOS
.OPTION ABSMOS
Syntax
.OPTION ABSMOS=x
Description
Current error tolerance (for MOSFET devices) in DC or transient analysis. The
ABSMOS setting determines whether the drain-to-source current solution has
converged. The drain-to-source current converged if:
■
The difference between the drain-to-source current in the last iteration,
versus the present iteration, is less than ABSMOS, or
■
This difference is greater than ABSMOS, but the percent change is less than
RELMOS.
If other accuracy tolerances also indicate convergence, HSPICE or HSPICE
RF solves the circuit at that timepoint, and calculates the next timepoint
solution. For low-power circuits, optimization, and single transistor simulations,
set ABSMOS = 1e-12. Default is 1e-6 (amperes).
See Also
.DC
.OPTION RELMOS
.TRAN
HSPICE® Command Reference
X-2005.09
197
3: Options in HSPICE Netlists
.OPTION ABSTOL
.OPTION ABSTOL
Syntax
.OPTION ABSTOL=x
Description
Sets the absolute error tolerance for branch currents for DC and transient
analysis. Decrease ABSTOL, if accuracy is more important than convergence
time. ABSTOL is the same as ABSI.
See Also
.DC
.OPTION ABSI
.TRAN
198
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ABSV
.OPTION ABSV
Syntax
.OPTION ABSV=x
Description
Sets 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 microvolts, 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 millivolts. The default
is 50 (microvolts).
You can use ABSV in HSPICE, but not HSPICE RF.
See Also
.DC
.OPTION VNTOL
.TRAN
HSPICE® Command Reference
X-2005.09
199
3: Options in HSPICE Netlists
.OPTION ABSVAR
.OPTION ABSVAR
Syntax
.OPTION ABSVAR=x
Description
Sets 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, then HSPICE discards the
solution, sets the timestep to a smaller value, and recalculates the solution.
This is called a timestep reversal. The default is 0.5 (volts).
For additional information, see section “DVDT Dynamic Timestep Algorithm” in
the HSPICE Simulation and Analysis User Guide.
You can use ABSVAR in HSPICE, but not in HSPICE RF.
See Also
.OPTION DVDT
200
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ABSVDC
.OPTION ABSVDC
Syntax
.OPTION ABSVDC=x
Description
Sets the minimum voltage for DC and transient analysis. If accuracy is more
critical than convergence, decrease ABSVDC. If you need voltages less than 50
micro-volts, 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 1000volt circuits, a reasonable value is 5 to 50 millivolts.
The default is the .OPTION VNTOL setting (VNTOL default = 50 mV).
See Also
.DC
.OPTION VNTOL
.TRAN
HSPICE® Command Reference
X-2005.09
201
3: Options in HSPICE Netlists
.OPTION ACCT
.OPTION ACCT
Syntax
.OPTION ACCT
.OPTION ACCT=[1|2]
Example 1
.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 was 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.
Description
The ACCT option in HSPICE generates a detailed accounting report.
Argument
Definition
.OPTION ACCT
Enables reporting.
.OPTION
ACCT = 1 (default)
Is the same as ACCT, without arguments.
.OPTION
ACCT = 2
Enables reporting, and matrix statistic reporting.
See Also
.DC
.TRAN
202
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ACCURATE
.OPTION ACCURATE
Syntax
.OPTION ACCURATE=x
Description
Selects 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 or
HSPICE RF. When set to 1, this option sets these control options:
LVLTIM =
DVDT = 2
RELVAR =
ABSVAR =
FT = 0.2
RELMOS =
3
0.2
0.2
0.01
The default is 0.
See Also
.OPTION ABSVAR
.OPTION DVDT
.OPTION FT
.OPTION LVLTIM
.OPTION RELMOS
.OPTION RELVAR
HSPICE® Command Reference
X-2005.09
203
3: Options in HSPICE Netlists
.OPTION ACOUT
.OPTION ACOUT
Syntax
.OPTION ACOUT=x
Description
AC output calculation method for the difference in values of magnitude, phase,
and decibels. Use these values for prints and plots. The default is 1.
The default (ACOUT = 1) selects the HSPICE method, which calculates the
difference of the magnitudes of the values. The SPICE method, ACOUT = 0,
calculates the magnitude of the differences in HSPICE.
You can use this option in HSPICE, but not in HSPICE RF.
204
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ALT999 or ALT9999
.OPTION ALT999 or ALT9999
Syntax
.OPTION ALT999
.OPTION ALT9999
Description
This option was developed to allow the.GRAPH statement to create more
output files when you ran .ALTER simulations.
This option is obsolete starting with version 2003.09. Without this option,
HSPICE can now generate up to 10,000 unique files.
See Also
.ALTER
.GRAPH
HSPICE® Command Reference
X-2005.09
205
3: Options in HSPICE Netlists
OPTION ALTCC
OPTION ALTCC
Syntax
.OPTION ALTCC=x
Description
Enables HSPICE to only read the input netlist once for multiple .ALTER
statements.
ALTCC = 1 enables reading input netlist only once for multiple .ALTER
statements.
ALTCC = 0 or -1 disables : HSPICE or HSPICE RF does not output a warning
message during transient analysis. HSPICE or HSPICE RF outputs the results,
after this transient analysis.
Note: You can use .OPTION ALTCC or .OPTION ALTCC=1 to ignore parsing
of an input netlist before an .ALTER statement in the process of standard
cell library characterization only when an .ALTER statement changes
parameters, source stimulus, analysis, or passive elements. Otherwise, this
option is ignored.
See Also
.ALTER
206
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ALTCHK
.OPTION ALTCHK
Syntax
.OPTION ALTCHK=x
Description
By default, HSPICE automatically reports topology errors in the latest elements
in your top-level netlist. It also reports errors in elements that you redefine by
using the .ALTER statement (altered netlist).
To disable topology checking in redefined elements (that is, to check topology
only in the top-level netlist, but not in the altered netlist), set:
.option altchk=0
By default, .OPTION ALTCHK is set to 1:
.option altchk=1
.option altchk
This enables topology checking in elements that you redefine using
the .ALTER statement. HSPICE RF does not support .ALTER statements.
See Also
.ALTER
HSPICE® Command Reference
X-2005.09
207
3: Options in HSPICE Netlists
.OPTION ARTIST
.OPTION ARTIST
Syntax
.OPTION ARTIST=x
Description
ARTIST = 2 enables the Cadence Analog Artist interface. This option requires
a specific license.
208
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ASPEC
.OPTION ASPEC
Syntax
.OPTION ASPEC=x
Description
Sets HSPICE or HSPICE RF to ASPEC-compatibility mode. When you set this
option, the simulator reads ASPEC models and netlists, and the results are
compatible. The default is 0 (HSPICE mode).
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
statement. The default (WL=0) assigns the length first, then the width.
See Also
.OPTION SCALE
.OPTION SCALM
.OPTION WL
HSPICE® Command Reference
X-2005.09
209
3: Options in HSPICE Netlists
.OPTION AUTOSTOP
.OPTION AUTOSTOP
Syntax
.OPTION AUTOSTOP
-or.OPTION AUTOSTOP=’expression’
Example
.option autostop='m1&&m2||m4'
.meas tran m1 trig v(bd_a0)
val='ddv/2'
fall=1
targ v(re_bd)
val='ddv/2'
rise=1
.meas tran m2 trig v(bd_a0)
val='ddv/2'
fall=2
targ v(re_bd)
val='ddv/2'
rise=2
.meas tran m3 trig v(bd_a0)
val='ddv/2'
rise=2
targ v(re_bd)
val='ddv/2'
rise=3
.meas tran m4 trig v(bd_a0)
val='ddv/2'
fall=3
targ v(re_bd)
val='ddv/2'
rise=4
.meas tran m5 trig v(bd_a0)
val='ddv/2' rise=3
targ
v(re_bd)
val='ddv/2'
rise=5
In this example, when either m1 and m2 are obtained, or just m4 is obtained,
the transient analysis ends.
Description
Stops a transient analysis in HSPICE or HSPICE RF, 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
statements succeeds, even if the others are not completed.
Also terminates the simulation, after completing all .MEASURE statements. This
is of special interest when testing corners.
See Also
.MEASURE
210
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION BADCHR
.OPTION BADCHR
Syntax
.OPTION BADCHR
Description
Generates a warning, if it finds a non-printable character in an input file.
HSPICE® Command Reference
X-2005.09
211
3: Options in HSPICE Netlists
.OPTION BEEP
.OPTION BEEP
Syntax
.OPTION BEEP=x
Description
BEEP = 1 sounds an audible tone when simulation returns a message, such
as:
info: HSPICE job completed.
BEEP = 0 turns off the audible tone.
212
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION BIASFILE
.OPTION BIASFILE
Syntax
.OPTION BIASFILE=x
Example
OPTION BIASFILE=’biaschk/mos.bias’
Description
If you use this option, HSPICE or HSPICE RF outputs the results of
all .BIASCHK commands to a file that you specify. If you do not set this option,
HSPICE or HSPICE RF outputs the .BIASCHK results to the *.lis file.
See Also
.BIASCHK
HSPICE® Command Reference
X-2005.09
213
3: Options in HSPICE Netlists
.OPTION BIAWARN
.OPTION BIAWARN
Syntax
.OPTION BIAWARN=x
Example
.OPTION BIAWARN=1
Description
BIAWARN = 1: HSPICE or HSPICE RF immediately outputs a warning
message when any local max bias voltage exceeds the limit during transient
analysis. After this transient analysis, HSPICE or HSPICE RF outputs the
results summary as filtered by noise.
BIAWARN = 0 (default): HSPICE or HSPICE RF does not output a warning
message during transient analysis. HSPICE or HSPICE RF outputs the results,
after this transient analysis.
See Also
.TRAN
214
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION BINPRINT
.OPTION BINPRINT
Syntax
.OPTION BINPRINT
Description
Outputs the binning parameters of the CMI MOSFET model. Currently
available only for Level 57.
HSPICE® Command Reference
X-2005.09
215
3: Options in HSPICE Netlists
.OPTION BKPSIZ
.OPTION BKPSIZ
Syntax
.OPTION BKPSIZ=x
Description
Sets the size of the breakpoint table. The default is 5000. This is an old option,
provided only for backward-compatibility.
216
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION BRIEF
.OPTION BRIEF
Syntax
.OPTION BRIEF=x
Description
Stops printback of the data file, until HSPICE or HSPICE RF finds an .OPTION
BRIEF = 0 or the .END statement. It also resets the LIST, NODE, and OPTS
options, and sets NOMOD. BRIEF = 0 enables printback. The NXX option is the
same as BRIEF.
See Also
.END
.OPTION LIST
.OPTION NODE
.OPTION NXX
.OPTION OPTS
HSPICE® Command Reference
X-2005.09
217
3: Options in HSPICE Netlists
.OPTION BYPASS
.OPTION BYPASS
Syntax
.OPTION BYPASS=x
Description
Bypasses model evaluations, if the terminal voltages do not change. Can be 0
(off), 1 (on), or 2 (applies to BSIM3v3 and BSIM4 in special cases). To speedup simulation, this option does not update the status of latent devices. To
enable bypassing, set .OPTION BYPASS = 1 for MOSFETs, MESFETs,
JFETs, BJTs, or diodes. Default = 1.
Use the BYPASS algorithm cautiously. Some circuit types might not converge,
and might lose accuracy in transient analysis and operating-point calculations.
218
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION BYTOL
.OPTION BYTOL
Syntax
.OPTION BYTOL=x
Description
Specifies 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.
You can use this option in HSPICE, but not in HSPICE RF.
See Also
.OPTION MBYPASS
.OPTION VNTOL
HSPICE® Command Reference
X-2005.09
219
3: Options in HSPICE Netlists
.OPTION CAPTAB
.OPTION CAPTAB
Syntax
.OPTION CAPTAB
Description
Prints table of single-plate node capacitances for diodes, BJTs, MOSFETs,
JFETs, and passive capacitors, at each operating point.
220
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION CDS
.OPTION CDS
Syntax
.OPTION CDS=x
Description
CDS = 2 produces a Cadence WSF (ASCII format) post-analysis file for
Opus. This option requires a specific license. The CDS option is the same as
the SDA option.
See Also
.OPTION SDA
HSPICE® Command Reference
X-2005.09
221
3: Options in HSPICE Netlists
.OPTION CHGTOL
.OPTION CHGTOL
Syntax
.OPTION CHGTOL=x
Description
Sets 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).
See Also
.OPTION CHGTOL
.OPTION LVLTIM
.OPTION RELQ
222
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION CMIFLAG
.OPTION CMIFLAG
Syntax
.OPTION CMIFLAG
Description
This option signals to load the dynamically-linked Common Model Interface
(CMI) library, libCMImodel.
See Also
.OPTION CUSTCMI
HSPICE® Command Reference
X-2005.09
223
3: Options in HSPICE Netlists
.OPTION CO
.OPTION CO
Syntax
.OPTION CO=<column_width>
Example
* Narrow print-out (default)
.OPTION CO=80
* Wide print-out
.OPTION CO=132
Description
The number of output variables that print on a single line of output, is a function
of the number of columns. Use .OPTION CO to set the column width for printouts in HSPICE.
HSPICE RF does not support the .OPTION CO statement.
You can set up to five output variables per 80-column output, and up to eight
output variables per 132-column output withtwelve characters per column.
HSPICE automatically creates additional print statements and tables for all
output variables beyond the number that the CO option specifies. The default is
80.
Argument
Definition
column_width
The number of characters in a single line of output.
See Also
.WIDTH
224
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION CONVERGE
.OPTION CONVERGE
Syntax
.OPTION CONVERGE=x
Description
Invokes different methods to solve non-convergence problems.
■
CONVERGE = -1 : Use with DCON = -1 to disable autoconvergence.
■
CONVERGE = 0 : Autoconvergence (default).
■
CONVERGE = 1 : Uses 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 : Uses a combination of DCSTEP and GMINDC ramping. Not
used in the autoconvergence flow.
■
CONVERGE = 3 : Invokes the source-stepping method. Not used in the
autoconvergence flow.
■
CONVERGE = 4 : Uses the gmath ramping method.
Even you did not set it in an .OPTION statement, the CONVERGE option
activates if a matrix floating-point overflows, or if HSPICE or HSPICE RF
reports a timestep too small error. The default is 0.
If a matrix floating-point overflows, then CONVERGE = 1.
See Also
.OPTION DCON
.OPTION DCSTEP
.OPTION DCTRAN
.OPTION GMINDC
HSPICE® Command Reference
X-2005.09
225
3: Options in HSPICE Netlists
.OPTION CPTIME
.OPTION CPTIME
Syntax
.OPTION CPTIME=x
Description
Sets 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 will take, especially when you debug new
data files. Default is 1e7 (400 days).
See Also
.OPTION LIMTIM
226
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION CSDF
.OPTION CSDF
Syntax
.OPTION CSDF=x
Description
Selects Common Simulation Data Format (Viewlogic-compatible graph data file
format).
HSPICE® Command Reference
X-2005.09
227
3: Options in HSPICE Netlists
.OPTION CSHDC
.OPTION CSHDC
Syntax
.OPTION CSHDC=x
Description
The same option as CSHUNT; use only with the CONVERGE option.
You can use the CSHDC option in HSPICE, but not in HSPICE RF.
See Also
.OPTION CONVERGE
.OPTION CSHUNT
228
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION CSHUNT
.OPTION CSHUNT
Syntax
.OPTION CSHUNT=x
Description
Capacitance added from each node to ground in HSPICE or HSPICE RF. Add
a small CSHUNT to each node to solve internal timestep too small problems,
caused by high-frequency oscillations or numerical noise. The default is 0.
HSPICE® Command Reference
X-2005.09
229
3: Options in HSPICE Netlists
.OPTION CUSTCMI
.OPTION CUSTCMI
Syntax
.OPTION CUSTCMI=x
Description
You set .OPTION CUSTCMI=1 jointly with .OPTION CMIFLAG to turn on gate
direct tunneling current modeling and instance parameter support for customer
CMI. You set .OPTION CUSTCMI=0 to turn off that feature.
See Also
.OPTION CMIFLAG
230
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION CVTOL
.OPTION CVTOL
Syntax
.OPTION CVTOL=x
Description
Changes 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 MOSFETS” chapter of the HSPICE Elements
and Device Models Manual for explicit equations and discussion.
You can use the .OPTION CVTOL statement in HSPICE, but not in HSPICE
RF.
HSPICE® Command Reference
X-2005.09
231
3: Options in HSPICE Netlists
.OPTION D_IBIS
.OPTION D_IBIS
Syntax
.OPTION D_IBIS=’ibis_files_directory’
Example
.OPTION d_ibis='/home/user/ibis/models'
Description
The .OPTION D_IBIS option specifies the directory containing the IBIS files. If
you specify several directories, then 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 .OPTION D_IBIS in the order that .OPTION
cards appear in the netlist. You can use the D_IBIS option to specify up to four
directories.
232
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DCAP
.OPTION DCAP
Syntax
.OPTION DCAP
Description
Selects equations, which HSPICE or HSPICE RF uses to calculate depletion
capacitance for Level 1 and 3 diodes, and BJTs. The HSPICE Elements and
Device Models Manual describes these equations.
HSPICE® Command Reference
X-2005.09
233
3: Options in HSPICE Netlists
.OPTION DCCAP
.OPTION DCCAP
Syntax
.OPTION DCCAP=x
Description
Generates 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 compacitance
values will not be evaluated and the printed value will be zero. The default is 0
(off).
See Also
.DC
234
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DCFOR
.OPTION DCFOR
Syntax
.OPTION DCFOR=x
Description
Use with .OPTION DCHOLD and the .NODESET statement to enhance DC
convergence.
DCFOR sets 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. The default is 0.
See Also
.DC
.NODESET
.OPTION DCHOLD
HSPICE® Command Reference
X-2005.09
235
3: Options in HSPICE Netlists
.OPTION DCHOLD
.OPTION DCHOLD
Syntax
.OPTION DCHOLD=x
Description
Use DCFOR and DCHOLD together to initialize DC analysis. You can use the
DCHOLD option in HSPICE, but not in HSPICE RF. DCFOR and DCHOLD
enhance the convergence properties of a DC simulation. DCFOR and DCHOLD
work with the .NODESET statement. The default is 1.
DCHOLD specifies how many iterations to hold a node, at the .NODESET voltage
values. 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 or
HSPICE RF ignores the values set in the .NODESET statement, and calculates
the DC solution by using the .NODESET fixed-source voltages open circuited.
See Also
.DC
.NODESET
.OPTION DCFOR
236
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DCIC
.OPTION DCIC
Syntax
.OPTION DCIC=x
Description
If DCIC=1 (default), each point in a DC sweep analysis acts like an operating
point and all .IC commands in the netlist are used.
If DCIC=0, .IC commands in the netlist are ignored for DC sweep analysis.
See Also
.IC
.DC
HSPICE® Command Reference
X-2005.09
237
3: Options in HSPICE Netlists
.OPTION DCON
.OPTION DCON
Syntax
.OPTION DCON=x
Description
If a circuit cannot converge, HSPICE or HSPICE RF 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
Vmax is the maximum voltage, and Imax is the maximum current.
■
If the circuit still cannot converge, HSPICE or HSPICE RF sets DCON = 2,
which sets DV = 1e6.
■
If the circuit uses discontinuous models or uninitialized flip-flops, simulation
might not converge. Set DCON = -1 and CONVERGE = -1 to disable
autoconvergence. HSPICE lists all non-convergent nodes and devices.
See Also
.OPTION CONVERGE
.OPTION DV
238
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DCSTEP
.OPTION DCSTEP
Syntax
.OPTION DCSTEP=x
Description
Converts 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. The default is 0 (seconds).
See Also
.DC
HSPICE® Command Reference
X-2005.09
239
3: Options in HSPICE Netlists
.OPTION DCTRAN
.OPTION DCTRAN
Syntax
.OPTION DCTRAN=x
Description
Invokes different methods to solve non-convergence problems. DCTRAN is an
alias for CONVERGE.
See Also
.OPTION CONVERGE
240
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DEFAD
.OPTION DEFAD
Syntax
.OPTION DEFAD=x
Description
The default MOSFET drain diode area in HSPICE. The default is 0.
HSPICE® Command Reference
X-2005.09
241
3: Options in HSPICE Netlists
.OPTION DEFAS
.OPTION DEFAS
Syntax
.OPTION DEFAS=x
Description
The default MOSFET source diode area in HSPICE. The default is 0.
242
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DEFL
.OPTION DEFL
Syntax
.OPTION DEFL=x
Description
The default MOSFET channel length in HSPICE. The default is 1e-4m.
HSPICE® Command Reference
X-2005.09
243
3: Options in HSPICE Netlists
.OPTION DEFNRD
.OPTION DEFNRD
Syntax
.OPTION DEFNRD=x
Description
The default number of squares for the drain resistor on a MOSFET. The default
is 0.
244
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DEFNRS
.OPTION DEFNRS
Syntax
.OPTION DEFNRS=x
Description
The default number of squares for the source resistor on a MOSFET. The
default is 0.
HSPICE® Command Reference
X-2005.09
245
3: Options in HSPICE Netlists
.OPTION DEFPD
.OPTION DEFPD
Syntax
.OPTION DEFPD=x
Description
The default MOSFET drain diode perimeter in HSPICE. The default is 0.
246
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DEFPS
.OPTION DEFPS
Syntax
.OPTION DEFPS=x
Description
The default MOSFET source diode perimeter in HSPICE. The default is 0.
HSPICE® Command Reference
X-2005.09
247
3: Options in HSPICE Netlists
.OPTION DEFW
.OPTION DEFW
Syntax
.OPTION DEFW=x
Description
The default MOSFET channel width in HSPICE. The default is 1e-4m.
248
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DELMAX
.OPTION DELMAX
Syntax
.OPTION DELMAX=x
Description
Sets the maximum Delta of the internal timestep. HSPICE automatically sets
the DELMAX value, based on timestep control factors. The initial DELMAX value,
shown in the HSPICE output listing, is generally not the value used for
simulation.
You can use the DELMAX option in HSPICE, but not in HSPICE RF.
HSPICE® Command Reference
X-2005.09
249
3: Options in HSPICE Netlists
.OPTION DI
.OPTION DI
Syntax
.OPTION DI=x
Description
Sets the maximum iteration-to-iteration current change, through voltagedefined branches (voltage sources and inductors). Use this option only if the
value of the ABSH control option is greater than 0. The default is 0.0.
See Also
.OPTION ABSH
250
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DIAGNOSTIC
.OPTION DIAGNOSTIC
Syntax
.OPTION DIAGNOSTIC
Description
Logs the occurrence of negative model conductances.
HSPICE® Command Reference
X-2005.09
251
3: Options in HSPICE Netlists
.OPTION DLENCSDF
.OPTION DLENCSDF
Syntax
.OPTION DLENCSDF=x
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, and the default is 5.
If you assign a floating decimal point, or if you specify less than 1 or more than
10 digits, HSPICE or HSPICE RF uses the default. For example, it places 5
digits to the right of a decimal point.
252
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DV
.OPTION DV
Syntax
.OPTION DV=x
Description
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 volt. The default is 1000 (or 1e6 if DCON = 2).
See Also
.DC
.OPTION DCON
.TRAN
HSPICE® Command Reference
X-2005.09
253
3: Options in HSPICE Netlists
.OPTION DVDT
.OPTION DVDT
Syntax
.OPTION DVDT=x
Description
Adjusts the timestep, based on rates of change for node voltage. The default is
4.
■
0 - original algorithm
■
1 - fast
■
2 - accurate
■
3,4 - balance speed and accuracy
■
You can use the DVDT option in HSPICE, but not in HSPICE RF. ACCURATE
also increases the accuracy of the results.
For additional information, see section “DVDT Dynamic Timestep Algorithm” in
the HSPICE Simulation and Analysis User Guide.
See Also
.OPTION ACCURATE
254
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION DVTR
.OPTION DVTR
Syntax
.OPTION DVTR=x
Description
Limits voltage in transient analysis. The default is 1000.
HSPICE® Command Reference
X-2005.09
255
3: Options in HSPICE Netlists
.OPTION EPSMIN
.OPTION EPSMIN
Syntax
.OPTION EPSMIN=x
Description
Specifies the smallest number that a computer can add or subtract, a constant
value. The default is 1e-28.
256
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION EXPLI
.OPTION EXPLI
Syntax
.OPTION EXPLI=x
Description
Current-explosion model parameter. PN junction characteristics, above the
explosion current, are linear. HSPICE or HSPICE RF determines the slope at
the explosion point. This improves simulation speed and convergence.
The default is 0.0 amp/AREAeff.
HSPICE® Command Reference
X-2005.09
257
3: Options in HSPICE Netlists
.OPTION EXPMAX
.OPTION EXPMAX
Syntax
.OPTION EXPMAX=x
Description
Specifies the largest exponent that you can use for an exponential, before
overflow occurs. Typical value for an IBM platform is 350.
258
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION FAST
.OPTION FAST
Syntax
.OPTION FAST
Description
Sets additional options, which increase simulation speed withminimal loss of
accuracy.
To speed-up simulation, this option does not update the status of latent
devices. Use this option for MOSFETs, MESFETs, JFETs, BJTs, and diodes.
The default is 0.
You can use FAST in HSPICE, but not HSPICE RF.
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 pre-processing time. Increasing the value of the MBYPASS or
BYTOL option, also helps simulations to run faster, but can reduce accuracy.
See Also
.OPTION BYTOL
.OPTION MBYPASS
.OPTION NOELCK
.OPTION NOTOP
HSPICE® Command Reference
X-2005.09
259
3: Options in HSPICE Netlists
.OPTION FFTOUT
.OPTION FFTOUT
Syntax
.OPTION FFTOUT=x
Description
Prints 30 harmonic fundamentals, sorted by size, THD, SNR, and SFDR, but
only if you specify a .OPTION FFTOUT statement and a .FFT freq=xxx
statement.
You can use the .OPTION FFTOUT statement in HSPICE, but not in HSPICE
RF.
See Also
.FFT
260
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION FS
.OPTION FS
Syntax
.OPTION FS=x
Description
Decreases 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 statement sets TSTEP. The default is 0.25.
You can use .OPTION FS in HSPICE, but not HSPICE RF.
See Also
.OPTION DELMAX
.OPTION DVDT
.TRAN
HSPICE® Command Reference
X-2005.09
261
3: Options in HSPICE Netlists
.OPTION FT
.OPTION FT
Syntax
.OPTION FT=x
Description
Decreases 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. The default is 0.25.
See Also
.OPTION DVDT
.TRAN
262
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION GDCPATH
.OPTION GDCPATH
Syntax
.OPTION GDCPATH[=x]
Description
Adds conductance to nodes having no DC path to ground. You use this option
to help solve no DC path to ground problems. If you specify GDCPATH in a
netlist without a value, that value is assumed to be 1e-15 (the default). The
default is 0 when not specified.
HSPICE® Command Reference
X-2005.09
263
3: Options in HSPICE Netlists
.OPTION GENK
.OPTION GENK
Syntax
.OPTION GENK=x
Description
Automatically computes second-order mutual inductance for several coupled
inductors. The default is 1, which enables the calculation.
264
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION GMAX
.OPTION GMAX
Syntax
.OPTION GMAX=x
Description
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. The default is 100 (mho).
You can use GMAX in HSPICE, but not in HSPICE RF.
See Also
.IC
.NODESET
HSPICE® Command Reference
X-2005.09
265
3: Options in HSPICE Netlists
.OPTION GMIN
.OPTION GMIN
Syntax
.OPTION GMIN=x
Description
Minimum conductance added to all PN junctions for a time sweep in transient
analysis. The default is 1e-12.
266
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION GMINDC
.OPTION GMINDC
Syntax
.OPTION GMINDC=x
Description
Conductance in parallel to all pn junctions and MOSFET nodes except gate for
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. The default is 1e-12.
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 or
HSPICE RF sets it to 1.0e-11. HSPICE or HSPICE RF manipulates GMINDC
in auto-converge mode.
See Also
.DC
.OPTION GRAMP
.OPTION PIVTOL
HSPICE® Command Reference
X-2005.09
267
3: Options in HSPICE Netlists
.OPTION GRAMP
.OPTION GRAMP
Syntax
.OPTION GRAMP=x
Description
HSPICE sets this value during auto-convergence (default is 0). Use GRAMP with
the GMINDC option to find the smallest GMINDC value that results in DC
convergence.
You can use GRAMP in HSPICE, but not HSPICE RF.
GRAMP specifies a conductance range, over which 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.
See Also
.DC
.OPTION GMINDC
268
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION GSHDC
.OPTION GSHDC
Syntax
.OPTION GSHDC=x
Description
Adds conductance from each node to ground when calculating the DC
operating point of the circuit (.OP). The default is 0.
You can use the GSHDC option in HSPICE, but not in HSPICE RF.
See Also
.OPTION GSHUNT
HSPICE® Command Reference
X-2005.09
269
3: Options in HSPICE Netlists
.OPTION GSHUNT
.OPTION GSHUNT
Syntax
.OPTION GSHUNT=x
Description
Adds conductance from each node to ground. The default is 0. Add a small
GSHUNT to each node to help solve Timestep too small problems caused by
either high-frequency oscillations or numerical noise.
You can use the GSHUNT option in HSPICE, but not in HSPICE RF.
270
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION H9007
.OPTION H9007
Syntax
.OPTION H9007
Description
Sets 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.
See Also
.OPTION EXPLI
HSPICE® Command Reference
X-2005.09
271
3: Options in HSPICE Netlists
.OPTION HIER_SCALE
.OPTION HIER_SCALE
Syntax
.OPTION HIER_SCALE=x
Description
If you set the HIER_SCALE option, you can use the S parameter to scale subcircuits.
272
■
0 interprets S as a user-defined parameter.
■
1 interprets S as a scale parameter.
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ICSWEEP
.OPTION ICSWEEP
Syntax
.OPTION ICSWEEP=x
Description
Saves the current analysis result of a parameter or temperature sweep as the
starting point in the next analysis in the sweep.
■
If ICSWEEP = 1 (default), the next analysis uses the current results.
■
If ICSWEEP = 0, the next analysis does not use the results of the current
analysis.
You can use ICSWEEP in HSPICE, but not in HSPICE RF.
HSPICE® Command Reference
X-2005.09
273
3: Options in HSPICE Netlists
.OPTION IMAX
.OPTION IMAX
Syntax
.OPTION IMAX=x
Description
Maximum timestep in timestep 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. HSPICE uses
the new timestep to calculate a new solution. IMAX also works with the IMIN
transient control option. IMAX is the same as ITL4. The default is 8.0.
You can use IMAX in HSPICE, but not HSPICE RF.
See Also
.OPTION FT
.OPTION IMIN
.OPTION ITL4
274
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION IMIN
.OPTION IMIN
Syntax
.OPTION IMIN=x
Description
Minimum timestep in timestep algorithms for transient analysis. IMIN is the
minimum number of iterations required to obtain convergence. 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. The default is 3.0.
You can use IMIN in HSPICE, but not HSPICE RF.
See Also
.OPTION IMAX
.OPTION ITL3
HSPICE® Command Reference
X-2005.09
275
3: Options in HSPICE Netlists
.OPTION INGOLD
.OPTION INGOLD
Syntax
.OPTION INGOLD=[0|1|2]
Example
.OPTION INGOLD=2
Description
By default, HSPICE or HSPICE RF prints variable values in engineering
notation:
F
P
N
U
=
=
=
=
1e-15
1e-12
1e-9
1e-6
M = 1e-3
K = 1e3
X = 1e6
G = 1e9
In contrast to exponential form, engineering notation provides two to three extra
significant digits, and aligns columns to facilitate comparison. To obtain output
in exponential form, specify .OPTION INGOLD = 1 or 2.
Argument
Definition
Defaults
INGOLD = 0
(default)
Engineering Format
1.234K
123M
INGOLD = 1
G Format (fixed and exponential)
1.234e+03
.123
INGOLD = 2
E Format (exponential SPICE)
1.234e+03
.123e-1
See Also
.OPTION MEASDGT
276
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION INTERP
.OPTION INTERP
Syntax
.OPTION INTERP=x
Description
Limits output for post-analysis tools, such as Cadence or Zuken, to only
the .TRAN timestep intervals. By default, HSPICE outputs all convergent
iterations. INTERP typically produces a much smaller design .tr# file.
Use INTERP = 1 with caution when the netlist includes .MEASURE statements.
To compute measure statements, HSPICE uses the post-processing output.
Reducing post-processing output can lead to interpolation errors in measure
results.
When you run data-driven transient analysis (.TRAN DATA) in an optimization
routine, HSPICE forces INTERP=1. HSPICE supports .TRAN DATA; HSPICE
RF does not. 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
.MEASURE
.OPTION ITRPRT
.TRAN
HSPICE® Command Reference
X-2005.09
277
3: Options in HSPICE Netlists
.OPTION ITL1
.OPTION ITL1
Syntax
.OPTION ITL1=x
Description
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, to converge, most models do not require more than 100
iterations. Set .OPTION ACCT to list how many iterations an operating point
requires. The default is 200.
See Also
.DC
.OPTION ACCT
278
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ITL2
.OPTION ITL2
Syntax
.OPTION ITL2=x
Description
Iteration limit for the DC transfer curve. Increasing this limit improves
convergence, only for very large circuits. Default is 50.
See Also
.DC
HSPICE® Command Reference
X-2005.09
279
3: Options in HSPICE Netlists
.OPTION ITL3
.OPTION ITL3
Syntax
.OPTION ITL3=x
Description
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. The default is 3.0.
You can use IMIN in HSPICE, but not HSPICE RF.
See Also
.OPTION IMAX
.OPTION IMIN
280
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ITL4
.OPTION ITL4
Syntax
.OPTION ITL4=x
Description
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. ITL4 is the same as IMAX. The default is 8.0.
You can use IMAX in HSPICE, but not HSPICE RF.
See Also
.OPTION FT
.OPTION IMAX
.OPTION IMIN
HSPICE® Command Reference
X-2005.09
281
3: Options in HSPICE Netlists
.OPTION ITL5
.OPTION ITL5
Syntax
.OPTION ITL5=x
Description
Sets an iteration limit for transient analysis. If a circuit uses more than ITL5
iterations, the program prints all results, up to that point. The default is 0.0.
allows an infinite number of iterations.
You can use the ITL5 option in HSPICE, but not in HSPICE RF.
282
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ITLPTRAN
.OPTION ITLPTRAN
Syntax
.OPTION ITLPTRAN=x
Description
Controls the iteration limit used in the final try of the pseudo-transient method in
OP or DC analysis. If simulation fails in the final try of the pseudo-transient
method, enlarge this option. The default is 30.
See Also
.DC
.OP
HSPICE® Command Reference
X-2005.09
283
3: Options in HSPICE Netlists
.OPTION ITLPZ
.OPTION ITLPZ
Syntax
.OPTION ITLPZ=x
Description
Sets the iteration limit for Pole/Zero analysis. The default is 100.
You can use ITLPZ in HSPICE, but not in HSPICE RF.
284
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ITRPRT
.OPTION ITRPRT
Syntax
.OPTION ITRPRT
Description
Prints output variables at their internal time points. This option might generate a
long output list.
HSPICE® Command Reference
X-2005.09
285
3: Options in HSPICE Netlists
.OPTION KCLTEST
.OPTION KCLTEST
Syntax
.OPTION KCLTEST=x
Description
Activates KCL (Kirchhoff’s Current Law) test. increases simulation time,
especially for large circuits, but very accurately checks the solution. The default
is 0.
If you set this value to 1, HSPICE or HSPICE RF 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
286
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION KLIM
.OPTION KLIM
Syntax
.OPTION KLIM=x
Description
This option sets 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. The default is 0.01.
HSPICE® Command Reference
X-2005.09
287
3: Options in HSPICE Netlists
.OPTION LENNAM
.OPTION LENNAM
Syntax
.OPTION LENNAM=x
Description
Maximum length of names in the printout of operating point analysis results.
Default is 8, and the maximum x value=1024.
288
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION LIMPTS
.OPTION LIMPTS
Syntax
.OPTION LIMPTS=x
Description
Number of points to print or plot in AC analysis. You do not need to set LIMPTS
for DC or transient analysis. HSPICE spools the output file to disk. The default
is 2001.
See Also
.AC
.DC
.TRAN
HSPICE® Command Reference
X-2005.09
289
3: Options in HSPICE Netlists
.OPTION LIMTIM
.OPTION LIMTIM
Syntax
.OPTION LIMTIM=x
Description
Amount of CPU time reserved to generate prints and plots, if a CPU time limit
(CPTIME = x) terminates simulation. The default is 2 (seconds), normally
sufficient for short printouts and plots.
See Also
.OPTION CPTIME
290
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION LIST
.OPTION LIST
Syntax
.OPTION LIST
Description
This option produces an element summary of the input data to print, and
calculates effective sizes of elements and the key values. The BRIEF option
suppresses the LIST option.
See Also
.OPTION BRIEF
.OPTION UNWRAP
.OPTION VFLOOR
HSPICE® Command Reference
X-2005.09
291
3: Options in HSPICE Netlists
.OPTION LVLTIM
.OPTION LVLTIM
Syntax
.OPTION LVLTIM=x
Description
Selects 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.
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.
See Also
.OPTION CHGTOL
.OPTION DVDT
.OPTION FS
.OPTION FT
.OPTION RELQ
292
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MAXAMP
.OPTION MAXAMP
Syntax
.OPTION MAXAMP=x
Description
Sets the maximum current, through voltage-defined branches (voltage sources
and inductors). If the current exceeds the MAXAMP value, HSPICE or HSPICE
RF reports an error. The default is 0.0.
HSPICE® Command Reference
X-2005.09
293
3: Options in HSPICE Netlists
.OPTION MAXORD
.OPTION MAXORD
Syntax
.OPTION MAXORD=x
Description
Maximum order of integration for the GEAR method in HSPICE. The x value
can be either 1 or 2.
■
MAXORD = 1 uses the backward Euler integration method.
■
MAXORD = 2 (default) is more stable, accurate, and practical.
See Also
.OPTION METHOD
294
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MBYPASS
.OPTION MBYPASS
Syntax
.OPTION MBYPASS=x
Description
Computes the default value of the BYTOL control option:
BYTOL = MBYPASSxVNTOL
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® Command Reference
X-2005.09
295
3: Options in HSPICE Netlists
.OPTION MCBRIEF
.OPTION MCBRIEF
Syntax
.OPTION MCBRIEF=x
Description
Controls how HSPICE outputs Monte Carlo parameters.
296
■
MCBRIEF=0: Outputs all Monte Carlo parameters (default)
■
MCBRIEF=1: Does not output the Monte Carlo parameters
■
MCBRIEF=2: Outputs the Monte Carlo parameters into a .lis file only.
■
MCBRIEF=3: Outputs the Monte Carlo parameters into the measure files
only.
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MEASDGT
.OPTION MEASDGT
Syntax
.OPTION MEASDGT=x
Description
Formats the .MEASURE statement output 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, although you can set it as high as
10. The default is 4.0.
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.
Use MEASDGT with .OPTION INGOLD=x to control the output data format.
See Also
.OPTION INGOLD
.MEASURE
HSPICE® Command Reference
X-2005.09
297
3: Options in HSPICE Netlists
.OPTION MEASFAIL
.OPTION MEASFAIL
Syntax
.OPTION MEASFAIL=0|1
Description
You can assign this option the following values:
■
MEASFAIL=0, outputs 0 into the .mt#, .ms#, or .ma# file, and prints failed to
the listing file.
■
MEASFAIL=1 (default), prints failed into the .mt#, .ms#, or .ma# file, and
into the listing file.
See Also
.MEASURE
298
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MEASFILE
.OPTION MEASFILE
Syntax
.OPTION MEASFILE=x
Description
Controls whether measure information outputs to single or multiple files when
an .ALTER statement is present in the netlist. You can assign this option the
following values:
■
MEASFILE=0, outputs measure information to several files.
■
MEASFILE=1 (default), outputs measure information to a single file.
See Also
.ALTER
.MEASURE
HSPICE® Command Reference
X-2005.09
299
3: Options in HSPICE Netlists
.OPTION MEASSORT
.OPTION MEASSORT
Syntax
.OPTION MEASSORT=x
Description
In versions of HSPICE before 2003.09, to automatically sort large numbers
of .MEASURE statements, you could use the .OPTION MEASSORT statement.
■
.OPTION MEASSORT=0 (default; did not sort .MEASURE statements).
■
.OPTION MEASSORT=1 (internally sorted .MEASURE statements).
You needed to set this option to 1 only if you used a large number of .MEASURE
statements, where you needed to list similar variables together (to reduce
simulation time). For a small number of .MEASURE statements, turning on
internal sorting sometimes slowed-down simulation while sorting, compared to
not sorting first.
Starting in version 2003.09, this option is obsolete. Now the measure
performance is order independent, and HSPICE ignores this option.
See Also
.MEASURE
300
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MEASOUT
.OPTION MEASOUT
Syntax
.OPTION MEASOUT=x
Description
This option outputs .MEASURE statement values and sweep parameters into an
ASCII file. Post-analysis processing (AvanWaves 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. The default is 1.
You can set this option to 0 (off) in the hspice.ini file.
See Also
.ALTER
.MEASURE
.TEMP
HSPICE® Command Reference
X-2005.09
301
3: Options in HSPICE Netlists
.OPTION MENTOR
.OPTION MENTOR
Syntax
.OPTION MENTOR=x
Description
MENTOR = 2 enables the Mentor MSPICE-compatible (ASCII) interface. This
option requires a specific license.
302
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION METHOD
.OPTION METHOD
Syntax
.OPTION METHOD=GEAR|TRAP
Description
Sets the numerical integration method for a transient analysis to either GEAR
or TRAP.
■
To use GEAR, set METHOD = GEAR, which sets LVLTIM = 2.
■
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 was 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. Default is TRAP (trapezoidal).
Gear algorithm:
OPTION METHOD = GEAR
Backward-Euler:
OPTION METHOD = GEAR MU = 0
Trapezoidal algorithm (default):
OPTION METHOD = TRAP
See Also
.OPTION LVLTIM
.OPTION MU
HSPICE® Command Reference
X-2005.09
303
3: Options in HSPICE Netlists
.OPTION MODMONTE
.OPTION MODMONTE
Syntax
.OPTION MODMONTE=x
Description
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 (default), 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.
304
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MODSRH
.OPTION MODSRH
Syntax
.OPTION MODSRH=x
Example
example.sp:
* modsrh used incorrectly
.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
This input file automatically searches for t6.inc. If t6.inc includes the nch model,
and you set MODSRH to 1, HSPICE or HSPICE RF does not load nch. Do not
set MODSRH=1 in this type of file call. Use this option in front of the .MODEL
card definition.
Description
If MODSRH=1, HSPICE or HSPICE RF does not load or reference a model
described in a .MODEL statement, if the netlist does not use that model. This
option shortens simulation run time when the netlist references many models,
but no element in the netlist calls those models. The default is MODSRH=0. If
MODSRH=1, then the read-in time increases slightly.
See Also
.MODEL
HSPICE® Command Reference
X-2005.09
305
3: Options in HSPICE Netlists
.OPTION MONTECON
.OPTION MONTECON
Syntax
.OPTION MONTECON=x
Description
Continues a Monte Carlo analysis in HSPICE (not supported in HSPICE RF).
Retrieves 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
analysis can use this Monte Carlo random value.
306
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION MU
.OPTION MU
Syntax
.OPTION MU=x
Description
This option defines the coefficient for trapezoidal integration. The value range is
0.0 to 0.5, and the default is 0.5.
HSPICE® Command Reference
X-2005.09
307
3: Options in HSPICE Netlists
.OPTION NEWTOL
.OPTION NEWTOL
Syntax
.OPTION NEWTOL=x
Description
Calculates 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. The default is 0.
You can use NEWTOL in HSPICE, but not in HSPICE RF.
308
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION NODE
.OPTION NODE
Syntax
.OPTION NODE=x
Example
1 M1:B D2:+ Q4:B
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.
Description
Prints 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:
+
B
B
C
D
E
G
S
S
Diode anode
Diode cathode
BJT base
MOSFET or JFET bulk
BJT collector
MOSFET or JFET drain
BJT emitter
MOSFET or JFET gate
BJT substrate
MOSFET or JFET source
See Also
.OPTION BRIEF
HSPICE® Command Reference
X-2005.09
309
3: Options in HSPICE Netlists
.OPTION NOELCK
.OPTION NOELCK
Syntax
.OPTION NOELCK
Description
No element check; bypasses element checking to reduce pre-processing time
for very large files.
310
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION NOISEMINFREQ
.OPTION NOISEMINFREQ
Syntax
.OPTION NOISEMINFREQ=x
Description
The .OPTION NOISEMINFREQ command option specifies the minimum
frequency of noise analysis. The default is 1e-5. If the frequency of noise
analysis is smaller than the minimum frequency, HSPICE automatically sets the
frequency for NOISEMINFREQ in noise analysis.
HSPICE® Command Reference
X-2005.09
311
3: Options in HSPICE Netlists
.OPTION NOMOD
.OPTION NOMOD
Syntax
.OPTION NOMOD
Description
Suppresses the printout of model parameters.
312
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION NOPAGE
.OPTION NOPAGE
Syntax
.OPTION NOPAGE
Description
Suppresses page ejects for title headings.
HSPICE® Command Reference
X-2005.09
313
3: Options in HSPICE Netlists
.OPTION NOPIV
.OPTION NOPIV
Syntax
.OPTION NOPIV=x
Description
Prevents HSPICE or HSPICE RF from automatically switching to pivoting
matrix factors, if a nodal conductance is less than PIVTOL. NOPIV inhibits
pivoting.
See Also
.OPTION PIVTOL
314
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION NOTOP
.OPTION NOTOP
Syntax
.OPTION NOTOP
Description
Suppresses topology checks to increase the speed for pre-processing very
large files.
HSPICE® Command Reference
X-2005.09
315
3: Options in HSPICE Netlists
.OPTION NOWARN
.OPTION NOWARN
Syntax
.OPTION NOWARN
Description
Suppresses all warning messages, except those generated from statements
in .ALTER blocks.
See Also
.ALTER
316
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION NUMDGT
.OPTION NUMDGT
Syntax
.OPTION NUMDGT=x
Description
This option controls the listing printout (.lis) accuracy. The value of x is typically
between 1 and 7, although you can set it as high as 10. The default is 4.0. This
option does not affect the accuracy of the simulation.
This option does affect the results files (ASCII and binary) if you use the
.OPTION POST_VERSION = 2001 setting. The default setting of results files
for printout accuracy is 5 digits.
See Also
.OPTION POST_VERSION
HSPICE® Command Reference
X-2005.09
317
3: Options in HSPICE Netlists
.OPTION NXX
.OPTION NXX
Syntax
.OPTION NXX
Description
Stops printback of the data file, until HSPICE or HSPICE RF finds
an .OPTION BRIEF=0 or the .END statement. 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
318
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION OFF
.OPTION OFF
Syntax
.OPTION OFF=x
Description
For all active devices, initializes terminal voltages to zero, if you did not initialize
them to other values. For example, if you did not initialize both drain and source
nodes of a transistor (using .NODESET, .IC statements, or connecting them
to sources), then OFF initializes all nodes of the transistor to 0.
HSPICE or HSPICE RF 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® Command Reference
X-2005.09
319
3: Options in HSPICE Netlists
.OPTION OPFILE
.OPTION OPFILE
Syntax
.OPTION OPFILE=value
Description
The OPFILE option outputs the operating point information to a file. value can
be 0 or 1.
320
■
If value is 1, operating point information is output to a file named
<design>.dp#.
■
If value is 0, the operating point information outputs to stdout.
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION OPTLST
.OPTION OPTLST
Syntax
.OPTION OPTLIST=x
Description
Outputs additional optimization information:
■
OPTLIST=0: No information (default).
■
OPTLIST=1: Prints parameter, Broyden update, and bisection results
information.
■
OPTLIST=2: Prints gradient, error, Hessian, and iteration information.
■
OPTLIST=3: Prints all of the above and Jacobian.
HSPICE® Command Reference
X-2005.09
321
3: Options in HSPICE Netlists
.OPTION OPTS
.OPTION OPTS
Syntax
.OPTION OPTS
Description
Prints 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.
See Also
.OPTION BRIEF
322
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION PARHIER
.OPTION PARHIER
Syntax
.OPTION PARHIER = < GLOBAL | LOCAL >
Example
.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
This example explicitly shows the difference between local and global scoping
for using parameters in sub-circuits.
Description
Use the .OPTION OPTLST parameter to specify scoping rules.
The default setting is GLOBAL.
See Also
.OPTION OPTLST
HSPICE® Command Reference
X-2005.09
323
3: Options in HSPICE Netlists
.OPTION PATHNUM
.OPTION PATHNUM
Syntax
.OPTION PATHNUM
Description
Prints subcircuit path numbers, instead of path names.
324
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION PIVOT
.OPTION PIVOT
Syntax
.OPTION PIVOT=x
Description
Selects a pivot algorithms. Use these algorithms to reduce simulation time, and
to achieve convergence in circuits that produce hard-to-solve matrix equations.
To select the pivot algorithm, set PIVOT as follows:
■
PIVOT=0: Original non-pivoting algorithm.
■
PIVOT=1: Original pivoting algorithm.
■
PIVOT=2: Picks the largest pivot in the row.
■
PIVOT=3: Picks the best pivot in a row.
■
PIVOT=10 (default): Fast, non-pivoting algorithm; requires more memory.
■
PIVOT=11: Fast, pivoting algorithm; requires more memory than PIVOT
values less than 11.
■
PIVOT=12: Picks the largest pivot in the row; requires more memory than
PIVOT values less than 12.
■
PIVOT=13: Fast, best pivot: faster; requires more memory than PIVOT
values less than 13.
The fastest algorithm is PIVOT = 13, which can improve simulation time up to
ten times, on very large circuits. However, PIVOT = 13 requires substantially
more memory for simulation.
Some circuits with large conductance ratios, such as switching regulator
circuits, might require pivoting.
If PIVTOL = 0, HSPICE or HSPICE RF automatically changes from nonpivoting to a row-pivot strategy, if it detects any diagonal-matrix entry less than
PIVTOL. This strategy provides the time and memory advantages of nonpivoting inversion, and avoids unstable simulations and incorrect results.
Use .OPTION NOPIV to prevent HSPICE or HSPICE RF from pivoting. For
very large circuits, PIVOT = 10, 11, 12, or 13, can require excessive memory.
If HSPICE or HSPICE RF switches to pivoting during a simulation, it displays
the message followed by the node numbers that cause the problem:
pivot change on the fly
HSPICE® Command Reference
X-2005.09
325
3: Options in HSPICE Netlists
.OPTION PIVOT
Use .OPTION NODE to cross-reference a node to an element. The SPARSE
option is the same as PIVOT.
See Also
.OPTION NODE
.OPTION NOPIV
.OPTION PIVREF
.OPTION PIVREL
.OPTION PIVTOL
.OPTION SPARSE
326
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION PIVREF
.OPTION PIVREF
Syntax
.OPTION PIVREF=x
Description
Pivot reference. Use PIVREF in PIVOT = 11, 12, or 13 to limit the size of the
matrix. The default is 1e+8.
See Also
.OPTION PIVOT
HSPICE® Command Reference
X-2005.09
327
3: Options in HSPICE Netlists
.OPTION PIVREL
.OPTION PIVREL
Syntax
.OPTION PIVREL=x
Description
Sets 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. If the value is too small, however, 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-20 (max = 1e-20, min = 1).
See Also
.OPTION PIVOT
328
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION PIVTOL
.OPTION PIVTOL
Syntax
.OPTION PIVTOL=x
Description
Absolute minimum value for which HSPICE or HSPICE RF accepts a matrix
entry as a pivot. If PIVOT=0, PIVTOL is the minimum conductance in the
matrix. The default is 1.0e-15.
PIVTOL must be less than GMIN or GMINDC. Values that approach 1 increase
the pivot.
See Also
.OPTION GMIN
.OPTION GMINDC
.OPTION PIVOT
HSPICE® Command Reference
X-2005.09
329
3: Options in HSPICE Netlists
.OPTION PLIM
.OPTION PLIM
Syntax
.OPTION PLIM
Description
Specifies 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 in HSPICE, which create a separate scale and
axis for each plot variable
You can use SPICE-compatibility mode in HSPICE, but not in HSPICE RF.
This option does not affect postprocessing of graph data.
330
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION POST
.OPTION POST
Syntax
.OPTION POST=[0|1|2|3|ASCII|BINARY]
Example
.OPTION POST=2
Description
Use an .OPTION POST statement to display high-resolution AvanWaves plots
of simulation results, on either a graphics terminal or a high-resolution laser
printer. Use .OPTION POST to provide output, without specifying other
parameters. POST has defaults, which supply usable data to most parameters.
■
POST = 0: Does not output simulation results.
■
POST = 1, BINARY: (Default) Output format is binary.
■
POST = 2, ASCII: Output format is ASCII.
■
POST = 3: Output format is New Wave binary.
See Also
.OPTION POST_VERSION
HSPICE® Command Reference
X-2005.09
331
3: Options in HSPICE Netlists
.OPTION POSTLVL
.OPTION POSTLVL
Syntax
.OPTION POSTLVL=x
Example
.OPTION POSTLVL=2
This example limits the data written to the waveform file to only the secondlevel nodes.
Description
The .OPTION POSTLVL option limits the data to only the x level nodes, which
is written to your waveform file.
332
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION POST_VERSION
.OPTION POST_VERSION
Syntax
.OPTION POST_VERSION=x
Description
Sets 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 (default) sets the node name length for the output file consistent
with the input restrictions (1024 characters), and limits the number of output
variables to 9999.
■
x = 2001 shows the new output file header, which includes the right
number of output variables rather than **** when the number exceeds 9999.
This option also changes the number of digits precision in results files to
match the value of .OPTION NUMDGT (when < 5).
If you set .OPTION POST_VERSION = 2001 POST= 2 in the netlist, then
HSPICE or HSPICE RF returns more-accurate ASCII results.
.option post_version=2001
To use binary values (with double precision) in the output file, include the
following in the input file:
*******************************************
.option post (or post=1) post_version=2001
*******************************************
For more accurate simulation results, comment this format.
See Also
.OPTION NUMDGT
.OPTION POST
HSPICE® Command Reference
X-2005.09
333
3: Options in HSPICE Netlists
.OPTION POSTTOP
.OPTION POSTTOP
Syntax
.OPTION POSTTOP=n
Example
POSTTOP = 1
This example limits the data written to the waveform file to only the top-level
nodes.
Description
The .OPTION POSTTOP option limits the data to only the data from the top n
level nodes, which is written to your waveform file. If you do not specify either
the .OPTION PROBE or the .OPTION POSTTOP options, then HSPICE outputs
all levels.
To enable the waveform display interface, you also need the .OPTION POST
option.
See Also
.OPTION POST
.OPTION PROBE
334
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION PROBE
.OPTION PROBE
Syntax
.OPTION PROBE=x
Description
Limits post-analysis output to only variables specified
in .PROBE, .PRINT, .PLOT, and .GRAPH statements. HSPICE RF
supports .PROBE and .PRINT statements, but does not support .PLOT
and .GRAPH statements. By default, HSPICE or HSPICE RF outputs all
voltages and power supply currents in addition to variables listed in .PROBE,
.PRINT, .PLOT, and .GRAPH statements. PROBE significantly decreases the
size of simulation output files.
See Also
.GRAPH
.PLOT
.PRINT
.PROBE
HSPICE® Command Reference
X-2005.09
335
3: Options in HSPICE Netlists
.OPTION PSF
.OPTION PSF
Syntax
.OPTION PSF=x
Description
Specifies whether HSPICE or HSPICE RF outputs binary or ASCII data when
you run an HSPICE simulation from Cadence Analog Artist.
The value of x can be 1 or 2.
■
If x is 2, HSPICE or HSPICE RF produces ASCII output.
■
If .OPTION ARTIST PSF = 1, HSPICE produces binary output.
See Also
.OPTION ARTIST
336
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION PURETP
.OPTION PURETP
Syntax
.OPTION PURETP=x
Description
Integration method to use for reversal time point. The default is 0. If you set
PURETP=1, then if HSPICE finds non-convergence, it uses TRAP (instead of
B.E) for the reversed time point. Use this option with the method=TRAP
statement to help some oscillating circuits to oscillate, if the default simulation
process cannot satisfy the result.
HSPICE® Command Reference
X-2005.09
337
3: Options in HSPICE Netlists
.OPTION PUTMEAS
.OPTION PUTMEAS
Syntax
.OPTION PUTMEAS=0|1
Description
The .OPTION PUTMEAS option controls the output variables, listed in
the .MEASURE statement.
■
0: Does not save variable values, which are listed in the .MEASURE
statement, 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, which are listed in the .MEASURE
statement, into the corresponding output file (such as .tr#, .ac# or .sw#).
This option is similar to the output of HSPICE 2000.4.
See Also
.MEASURE
338
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RELH
.OPTION RELH
Syntax
.OPTION RELH=x
Description
Relative current tolerance, through voltage-defined branches (voltage sources
and inductors). Use RELH to check current convergence, but only if the value of
the ABSH control option is greater than zero. The default is 0.05.
You can use RELH in HSPICE, but not in HSPICE RF.
See Also
.OPTION ABSH
HSPICE® Command Reference
X-2005.09
339
3: Options in HSPICE Netlists
.OPTION RELI
.OPTION RELI
Syntax
.OPTION RELI=x
Description
Sets the relative error/tolerance change, from iteration to iteration. This
parameter determines convergence for all currents in diode, BJT, and JFET
devices. (RELMOS sets tolerance for MOSFETs). This 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
340
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RELMOS
.OPTION RELMOS
Syntax
.OPTION RELMOS=x
Description
Sets the relative error tolerance (percent) for drain-to-source current, from
iteration-to-iteration. This parameter determines convergence for currents in
MOSFET devices. (.OPTION RELI sets the tolerance for other active devices.)
Sets the change in current, from the value calculated at the previous timepoint.
HSPICE or HSPICE RF uses the .OPTION RELMOS value, only if the current is
greater than the .OPTION ABSMOS floor value. The default is 0.05.
See Also
.OPTION ABSMOS
.OPTION RELI
.OPTION RELMOS
HSPICE® Command Reference
X-2005.09
341
3: Options in HSPICE Netlists
.OPTION RELQ
.OPTION RELQ
Syntax
.OPTION RELQ=x
Description
Used in the timestep algorithm for local truncation error (LVLTIM = 2). RELQ
changes the timestep size. 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.
You can use RELQ in HSPICE, but not in HSPICE RF.
See Also
.OPTION LVLTIM
342
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RELTOL
.OPTION RELTOL
Syntax
.OPTION RELTOL=x
Description
Relative error tolerance for voltages. Use RELTOL with the ABSV control option
to determine voltage convergence. Increasing RELTOL increases the relative
error. RELTOL is the same as RELV. RELI and RELVDC options default to the
RELTOL value. The default is 1e-3.
You can use the RELTOL and RELV options in HSPICE, but not in HSPICE RF.
See Also
.OPTION ABSV
.OPTION RELI
.OPTION RELV
.OPTION RELVDC
HSPICE® Command Reference
X-2005.09
343
3: Options in HSPICE Netlists
.OPTION RELV
.OPTION RELV
Syntax
.OPTION RELV=x
Description
Sets the relative error tolerance for voltages. If voltage or current exceeds the
absolute tolerances, a RELV test determines convergence. Increasing RELV
increases the relative error. You should generally maintain RELV at its default
value. RELV conserves simulator charge. For voltages, RELV is the same as
RELTOL. The default is 1e-3.
See Also
.OPTION RELTOL
344
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RELVAR
.OPTION RELVAR
Syntax
.OPTION RELVAR=x
Description
Use this option with ABSVAR, and the DVDT timestep algorithm. RELVAR sets
the relative voltage change for LVLTIM = 1 or 3. If the node voltage at the
current time point exceeds the node voltage at the previous time point by
RELVAR, then HSPICE reduces the timestep, and calculates a new solution at
a new time point. The default is 0.30 (30%).
For additional information, see section “DVDT Dynamic Timestep Algorithm” in
the HSPICE Simulation and Analysis User Guide.
You can use the RELVAR option in HSPICE, but not in HSPICE RF.
See Also
.OPTION ABSVAR
.OPTION DVDT
.OPTION LVLTIM
HSPICE® Command Reference
X-2005.09
345
3: Options in HSPICE Netlists
.OPTION RELVDC
.OPTION RELVDC
Syntax
.OPTION RELVDC=x
Description
Sets the relative error tolerance for voltages. If voltages or currents exceed their
absolute tolerances, the RELVDC test determines convergence. Increasing
RELVDC increases the relative error. You should generally maintain RELVDC at
its default value. RELVDC conserves simulator charge. Default is RELTOL
(RELTOL default = 1e-3).
See Also
.OPTION RELTOL
346
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RESMIN
.OPTION RESMIN
Syntax
.OPTION RESMIN=x
Description
Minimum resistance for all resistors, including parasitic and inductive
resistances. The default is 1e-5 (ohm), and the range is 1e-15 to 10 ohm.
HSPICE® Command Reference
X-2005.09
347
3: Options in HSPICE Netlists
.OPTION RISETIME
.OPTION RISETIME
Syntax
.OPTION RISETIME=x
Description
Smallest risetime of a signal. Use this option only in transmission line models
or HSPICE RF. In the U element, this equation determines the number of
lumps:
TDeff
MIN 20, 1 +  ---------------------------- ⋅ 20
RISETIME
TDeff is the end-to-end delay in a transmission line. The W element uses
RISETIME, only if Rs or Gd is non-zero. In such cases, RISETIME determines
the maximum signal frequency.
348
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RMAX
.OPTION RMAX
Syntax
.OPTION RMAX=x
Description
Sets 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.
The maximum value is 1e+9, the minimum value is 1e-9. The recommended
maximum value is 1e+5. Supported in HSPICE and HSPICE RF.
For a discussion about timestep control, see section “Timestep Control for
Accuracy” in the HSPICE Simulation and Analysis User Guide.
See Also
.OPTION DELMAX
.OPTION DVDT
.OPTION LVLTIM
HSPICE® Command Reference
X-2005.09
349
3: Options in HSPICE Netlists
.OPTION RMIN
.OPTION RMIN
Syntax
.OPTION RMIN=x
Description
Sets 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.
You can use RMIN in HSPICE, but not HSPICE RF.
See Also
.OPTION FT
.OPTION IMAX
350
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION RUNLVL
.OPTION RUNLVL
Syntax
.OPTION RUNLVL=x
Description
The value for the .OPTION RUNLVL option controls the speed and accuracy
trade-off. Higher values of RUNLVL result in higher accuracy and longer
simulation times, while lower values give lower accuracy and faster simulation
runtimes. The value of RUNLVL can be set to 0, 1, 2, 3, 4, 5, or 6.
The RUNLVL option setting controls the scaling of all simulator tolerances
simulatenously and affects timestep control, 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 in order to meet
stricter error tolerances. The mode activated with RUNLVL affects only transient
analysis.
When RUNLVL is set to
■
0, the algorithm turns off.
■
1, the simulation runs at the lowest simulation runtime.
■
3, is the default value.
■
5 or 6, corresponds to the HSPICE standard accurate mode. For most
circuits, RUNLVL = 5 is similar to HSPICE standard accurate mode.
RUNLVL = 6 has the highest accuracy.
If .OPTION ACCURATE is specified in the netlist together with RUNLVL, then the
value of RUNLVL is limited to 5. In this case, specifying RUNLVL with a value
smaller than 5 results in simulation running with RUNLVL = 5.
The RUNLVL option interacts with other options as follows:
1. The RUNLVL option, regardless of its position in the netlist, overrides the
LVLTIM and DVDT timestep control mode options.
2. When RUNLVL is specified in the netlist, the default value of the BYPASS
option is 1. Setting BYPASS = 0 disables model bypass, regardless of the
order in which BYPASS and RUNLVL are set.
3. If .OPTION ACCURATE is set, then the RUNLVL value is limited to 5, and the
default value of BYPASS is set to 0. This behavior is independent of the
order of the RUNLVL, BYPASS, and ACCURATE options.
HSPICE® Command Reference
X-2005.09
351
3: Options in HSPICE Netlists
.OPTION RUNLVL
4. 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.
See Also
.OPTION ACCURATE
.OPTION BYPASS
.OPTION DVDT
.OPTION LVLTIM
.OPTION RELTOL
.TRAN
352
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION SCALE
.OPTION SCALE
Syntax
.OPTION SCALE=x
Description
Element scaling factor in HSPICE or HSPICE RF. Scales parameters in
element cards, by their value. The default is 1.
HSPICE® Command Reference
X-2005.09
353
3: Options in HSPICE Netlists
.OPTION SCALM
.OPTION SCALM
Syntax
.OPTION SCALM=x
Description
Model scaling factor in HSPICE or HSPICE RF. Scales model parameters by
their value. The default is 1. See the HSPICE Elements and Device Models
Manual for parameters this option scales.
354
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION SDA
.OPTION SDA
Syntax
.OPTION SDA=x
Description
SDA = 2 produces a Cadence WSF (ASCII format) post-analysis file for
Opus. This option requires a specific license. The SDA is the same as the CDS
option.
See Also
.OPTION CDS
HSPICE® Command Reference
X-2005.09
355
3: Options in HSPICE Netlists
.OPTION SEARCH
.OPTION SEARCH
Syntax
.OPTION SEARCH = ‘directory_path’
Example
.OPTION SEARCH = ‘$installdir/parts/vendor’
Description
Use the .OPTION SEARCH statement to automatically access a library.
This example searches for models in the vendor subdirectory, under the
<$installdir>/parts installation directory (see Figure 7). The parts/
directory contains the DDL subdirectories.
Figure 7
Vendor Library Usage
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
.model nch nmos level = 28
+ xl = vendor_xl ...
.macro buffer in out vdd vss
m1 out in vdd vdd nch w = 10 l = 1
...
Note: The ‘/usr’ directory is in the
HSPICE install directory.
356
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION SEED
.OPTION SEED
Syntax
.OPTION SEED=x
Description
Starting seed for random-number generator in HSPICE Monte Carlo analysis
(HSPICE RF does not support Monte Carlo analysis or the .OPTION SEED
statement). The minimum value is 1; the maximum value is 259200.
HSPICE® Command Reference
X-2005.09
357
3: Options in HSPICE Netlists
.OPTION SLOPETOL
.OPTION SLOPETOL
Syntax
.OPTION SLOPETOL=x
Description
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 or HSPICE RF ignores the breakpoint
for the point between the segments. The default is 0.75.
358
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION SPARSE
.OPTION SPARSE
Syntax
.OPTION SPARSE=x
Description
The SPARSE option is the same as PIVOT.
See Also
.OPTION PIVOT
HSPICE® Command Reference
X-2005.09
359
3: Options in HSPICE Netlists
.OPTION SPICE
.OPTION SPICE
Syntax
.OPTION SPICE=x
Example 1
Example of general parameters, used with .OPTION SPICE:
TNOM = 27 DEFNRD = 1
ACOUT = 0 DC
PIVOT PIVTOL = IE-13
ITL1 = 100
ABSMOS = 1E-6 RELMOS
VNTOL = 1E-6
ABSVDC = 1E-6 RELVDC
DEFNRS = 1 INGOLD = 2
PIVREL = 1E-3 RELTOL = 1E-3
= 1E-3 ABSTOL = 1E-12
= 1E-3 RELI = 1E-3
Example 2
Example of 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
Example 3
Example of 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
Description
Makes HSPICE compatible with Berkeley SPICE. HSPICE RF is C-based and
not Fortran-based so it is not compatible with Berkeley SPICE. You can
use .OPTION SPICE in HSPICE, but not in HSPICE RF. If you set this option,
HSPICE uses the options and model parameters explained in the examples.
360
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION SPMODEL
.OPTION SPMODEL
Syntax
.OPTION SPMODEL [= name]
Example 1
.option spmodel
This example disables the previous .OPTION VAMODEL, but has no effect on
the other VAMODEL options if they are specified for the individual cells. For
example, if .OPTION VAMODEL = vco has been set, the vco cell uses the
Verilog-A definition whenever it is available until .OPTION SPMODEL = vco
disables it.
Example 2
.option spmodel=chargepump
This example disables the previous .OPTION VAMODEL = chargepump,
which causes all instantiations of chargepump to now use the subcircuit
definition again.
Description
This option is for use in HSPICE with Verilog-A only. 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.
HSPICE® Command Reference
X-2005.09
361
3: Options in HSPICE Netlists
.OPTION STATFL
.OPTION STATFL
Syntax
.OPTION STATFL=x
Description
Controls whether HSPICE creates a .st0 file.
362
■
STATFL = 0 (default) outputs a .st0 file.
■
STATFL = 1 suppresses the .st0 file.
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION SYMB
.OPTION SYMB
Syntax
.OPTION SYMB=x
Description
If you set the SYMB option to 1, HSPICE operates with a symbolic operating
point algorithm to get initial guesses before calculating operating points. The
default is 0.
HSPICE® Command Reference
X-2005.09
363
3: Options in HSPICE Netlists
.OPTION TIMERES
.OPTION TIMERES
Syntax
.OPTION TIMERES=x
Description
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. The default is 1 ps.
You can use TIMERES in HSPICE, but not in HSPICE RF.
364
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION TNOM
.OPTION TNOM
Syntax
.OPTION TNOM=x
Description
Reference temperature for HSPICE or HSPICE RF simulation. At this
temperature, component derating is zero. The default is 25 °C. If you
enable .OPTION SPICE (HSPICE only; HSPICE RF does not support this
option), the default is 27 °C.
Note:
The reference temperature defaults to the analysis temperature if you do not
explicitly specify a reference temperature.
See Also
.OPTION SPICE
.TEMP
HSPICE® Command Reference
X-2005.09
365
3: Options in HSPICE Netlists
.OPTION TRCON
.OPTION TRCON
Syntax
.OPTION TRCON=x
Description
Controls the speed of some special circuits. For some large non-linear circuits
with large TSTOP/TSTEP values, analysis might run for an excessively long
time. In this case, HSPICE might automatically set a new and bigger RMAX
value to speed up the analysis for primary reference. In most cases, however,
HSPICE does not activate this type of autospeedup process.
For autospeedup to occur, all three of the following conditions must occur:
■
N1 (Number of Nodes) > 1,000
■
N2 (TSTOP/TSTEP) >= 10,000
■
N3 (Total Number of Diode, BJTs, JFETs and MOSFETs) > 300
Autospeedup is most likely to occur if the circuit also meets either of the
following conditions:
■
N2 >= 1e+8, and N3 > 500, or
■
N2 >= 2e+5, and N3 > 1e+4
■
TRCON = 3: enable auto-speedup only. HSPICE invokes auto-speed up if:
•
there are more than 1000 nodes, or
•
there are more than 300 active devices, or
•
Tstop/Tstep (as defined in .TRAN) > 1e8.
When auto-speedup is active, RMAX increases, and HSPICE can take larger
timesteps.
■
■
366
TRCON = 2: enables auto-convergence only.
•
HSPICE invokes auto-convergence if you use the default integration
method (trapezoidal), and if HPSICE fails to converge, an “internal
timestep too small” error is issued.
•
Auto-convergence sets METHOD = gear, LVLTIM = 2, and starts the
transient simulation again from time=0.
TRCON = 1: enables both auto-convergence and auto-speedup.
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION TRCON
■
TRCON = 0: disables both auto-convergence and auto-speedup (default).
■
TRCON = -1: same as TRCON = 0.
TRCON also controls the automatic convergence process (autoconvergence) as
well as the automatic speedup (autospeedup) processes in HSPICE. You
cannot use TRCON in HSPICE RF. HSPICE also uses autoconvergence in DC
analysis, if the Newton-Raphson (N-R) method fails to converge.
If the circuit fails to converge using the trapezoidal (TRAP) numerical
integration method (for example, because of trapezoidal oscillation), HSPICE
uses the GEAR method and LTE timestep algorithm to run the transient
analysis again from time=0. This process is called autoconvergence.
Autoconvergence sets options to their default values before the second try:
METHOD=GEAR, LVLTIM=2, MBYPASS=1.0,
+ BYPASS=0.0, SLOPETOL=0.5,
+ BYTOL= min{mbypas*vntol and reltol}
RMAX = 2.0 if it was 5.0 in the first run; otherwise RMAX does not change.
See Also
.OPTION BYPASS
.OPTION BYTOL
.OPTION MBYPASS
.OPTION RMAX
.OPTION SLOPETOL
HSPICE® Command Reference
X-2005.09
367
3: Options in HSPICE Netlists
.OPTION TRTOL
.OPTION TRTOL
Syntax
.OPTION TRTOL=x
Description
Used in the timestep algorithm for local truncation error (LVLTIM = 2).
HSPICE multiplies TRTOL by the internal timestep, which the timestep
algorithm for the local truncation error generates. 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 time-step 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. The default is 7.0.
You can use TRTOL in HSPICE, but not HSPICE RF.
See Also
.OPTION LVLTIM
368
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION UNWRAP
.OPTION UNWRAP
Syntax
.OPTION UNWRAP
Description
Displays phase results for AC analysis in unwrapped form (with a continuous
phase plot).HSPICE uses these results to accurately calculate group delay
(HSPICE RF does not support group time delays in AC analysis output). It also
uses unwrapped phase results to compute group delay, even if you do not set
UNWRAP.
HSPICE® Command Reference
X-2005.09
369
3: Options in HSPICE Netlists
.OPTION VAMODEL
.OPTION VAMODEL
Syntax
.OPTION VAMODEL [=name]
Example 1
.option vamodel=vco
This example specifies a Verilog-A definition for all instantiations of the cell
vco.
Example 2
.option vamodel=vco vamodel=chargepump
This example specifies a Verilog-A definition for all instantiations of the vco and
chargepump cells.
Example 3
.option vamodel
This example instructs HSPICE to always use the Verilog-A definition whenever
it is available.
Description
This option is for use in HSPICE with Verilog-A only. This option specifies that
the 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.
370
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION VERIFY
.OPTION VERIFY
Syntax
.OPTION VERIFY=x
Description
This option is an alias for .OPTION LIST.
See Also
.OPTION LIST
HSPICE® Command Reference
X-2005.09
371
3: Options in HSPICE Netlists
.OPTION VFLOOR
.OPTION VFLOOR
Syntax
.OPTION VFLOOR=x
Description
Minimum voltage to print in output listing. All voltages lower than VFLOOR, print
as 0. Affects only the output listing: VNTOL (ABSV) sets minimum voltage to use
in a simulation.
See Also
.OPTION ABSV
.OPTION VNTOL
372
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION VNTOL
.OPTION VNTOL
Syntax
.OPTION VNTOL=x
Description
The VNTOL option is the same as the ABSV option.
See Also
.OPTION ABSV
HSPICE® Command Reference
X-2005.09
373
3: Options in HSPICE Netlists
.OPTION WACC
.OPTION WACC
Syntax
.OPTION WACC=x
Description
This option is used to activate the dynamic step control algorithm for a W
element transient analysis. WACC is a non-negative real value, which can be set
between 0.0 and 10.0.
When WACC is positive, the dynamic step control algorithm is activated. Larger
values result in higher performance with lower accuracy, while smaller values
result in lower performance with better accuracy.
Use WACC = 1.0 for normal simulation and WACC = 0.1 for an accurate
simulation. When WACC = 0.0, the original step control method is used with
predetermined static breakpoints. Currently the default value is 0.0. For
HSPICE RF, the default value for WACC is 0.5. If WACC is set as 0.0, no control
is added.
374
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION WNFLAG
.OPTION WNFLAG
Syntax
.OPTION WNFLAG=[0|1]
Description
This option only applies to BSIM4 models. You use this option to select a bin
model.
When an .OPTION WNFLAG instance parameter
■
is not specified, the bin model specified by this option is used.
■
is specified, its value is used.
Use WNFLAG=1 (default) to select the bin model based on W (BSIM4 MOSFET
channel width) per NF (number of device fingers) parameters.
Use WNFLAG=0 to select the bin model based on total W.
HSPICE® Command Reference
X-2005.09
375
3: Options in HSPICE Netlists
.OPTION WARNLIMIT
.OPTION WARNLIMIT
Syntax
.OPTION WARNLIMIT=x
Description
Limits how many times certain warnings appear in the output listing. This
reduces the output listing file size. x is 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.
The default is 1.
376
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION WL
.OPTION WL
Syntax
.OPTION WL=x
Description
Reverses the order of the MOS element VSIZE. Default order is length-width;
changes the order to width-length. The default is 0.
HSPICE® Command Reference
X-2005.09
377
3: Options in HSPICE Netlists
.OPTION XDTEMP
.OPTION XDTEMP
Syntax
.OPTION XDTEMP=value
Example
.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. Finally, the DTEMP value of each element in this
example is:
Elements DTEMP Value (Celsius)
X1 2
X1.R1 2+3 =5
X1.C1 2
X2 2+4=6
X2.R2 6
Description
The .OPTION XDTEMP statement defines how HSPICE interprets the DTEMP
parameter, where value is either:
■
0 (the default), indicating a user-defined parameter, or
■
1 indicates a temperature difference parameter.
If you set .OPTION XDTEMP to 1, HSPICE adds the DTEMP value in the
subcircuit call statement to all elements within the subcircuit, that use the
DTEMP keyword syntax.
The DTEMP parameter is cumulative throughout the design hierarchy.
378
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
.OPTION ZUKEN
Syntax
.OPTION ZUKEN=x
Description
This option enables or disables the Zuken interface.
■
If x is 2, enables the Zuken interactive interface.
■
If x is 1 (default), disables this interface.
HSPICE® Command Reference
X-2005.09
379
3: Options in HSPICE Netlists
.OPTION ZUKEN
380
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
HSPICE® Command Reference
X-2005.09
381
3: Options in HSPICE Netlists
.OPTION ZUKEN
382
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
HSPICE® Command Reference
X-2005.09
383
3: Options in HSPICE Netlists
.OPTION ZUKEN
384
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
HSPICE® Command Reference
X-2005.09
385
3: Options in HSPICE Netlists
.OPTION ZUKEN
386
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
HSPICE® Command Reference
X-2005.09
387
3: Options in HSPICE Netlists
.OPTION ZUKEN
388
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
HSPICE® Command Reference
X-2005.09
389
3: Options in HSPICE Netlists
.OPTION ZUKEN
390
HSPICE® Command Reference
X-2005.09
3: Options in HSPICE Netlists
.OPTION ZUKEN
HSPICE® Command Reference
X-2005.09
391
3: Options in HSPICE Netlists
.OPTION ZUKEN
392
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
4
Commands in Digital Vector Files
4
Contains an alphabetical listing of the commands you can use in an
digital vector file.
You can use the following commands in a digital vector file.
ENABLE
TDELAY
VIL
IO
TFALL
VNAME
ODELAY
TRISE
VOH
OUT or OUTZ
TRIZ
VOL
PERIOD
TSKIP
VREF
RADIX
TUNIT
VTH
SLOPE
VIH
HSPICE® Command Reference
X-2005.09
393
4: Commands in Digital Vector Files
ENABLE
ENABLE
Syntax
ENABLE controlling_signalname mask
Argument
Definition
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.
Example
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.
■
The first enable statement 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.
Description
The ENABLE statement specifies the controlling signal(s) for bidirectional
signals. All bidirectional signals require an ENABLE statement. If you specify
more than one ENABLE statement, the last statement overrules the previous
statement, and HSPICE or HSPICE RF issues a warning message:
[Warning]:[line 6] resetting enable signal to WENB for bit ’XYZ’
394
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
IDELAY
IDELAY
Syntax
IDELAY delay_value mask
Argument
Definition
delay_value
Time delay to apply to the signals.
mask
Signals to which the delay applies. If you do not provide a mask, the
delay value applies to all signals.
Example
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 statement so HSPICE or HSPICE
RF uses the default, ns, as the time unit for this example. The first TDELAY
statement indicates that all signals have the same delay time of 1.0ns.
Subsequent TDELAY, IDELAY, or ODELAY statements 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.
Description
Defines an input delay time for bidirectional signals, relative to the absolute
time of each row in the Tabular Data section.
HSPICE or HSPICE RF ignores IDELAY settings on output signals, and issues
a warning message.
You can specify more than one TDELAY, IDELAY, or ODELAY statement.
HSPICE® Command Reference
X-2005.09
395
4: Commands in Digital Vector Files
IDELAY
■
If you apply more than one TDELAY (IDELAY, ODELAY) statement to a
signal, the last statement overrules the previous statements, and HSPICE
or HSPICE RF issues a warning.
■
If you do not specify the signal delays in a TDELAY, IDELAY, or ODELAY
statement, HSPICE or HSPICE RF defaults to zero.
See Also
ODELAY
TDELAY
TUNIT
396
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
IO
IO
Syntax
IO I | O | B | U
[I | O | B | U ...]
Argument
Definition
i
Input, which HSPICE or HSPICE RF uses to stimulate the circuit.
o
Expected output, which HSPICE or HSPICE RF compares with the
simulated outputs.
b
Bidirectional vector.
u
Unused vector, which HSPICE or HSPICE RF ignores.
Example
io i i i bbbb iiiioouu
Description
The IO statement defines 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 statement, HSPICE or HSPICE RF assumes
that all signals are input signals.
■
If you define more than one IO statement, the last statement overrules
previous statements.
HSPICE® Command Reference
X-2005.09
397
4: Commands in Digital Vector Files
ODELAY
ODELAY
Syntax
ODELAY delay_value mask
Argument
Definition
delay_value
Time delay to apply to the signals.
mask
Signals to which the delay applies. If you do not provide a mask,
the delay value applies to all signals.
Example
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 statement so HSPICE or HSPICE
RF uses the default, ns, as the time unit for this example. The first TDELAY
statement indicates that all signals have the same delay time of 1.0ns.
Subsequent TDELAY, IDELAY, or ODELAY statements 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.
Description
Defines an output delay time for bidirectional signals relative to the absolute
time of each row in the Tabular Data section.
HSPICE or HSPICE RF ignores ODELAY settings on input signals and issues a
warning message.
You can specify more than one TDELAY, IDELAY, or ODELAY statement.
398
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
ODELAY
■
If you apply more than one TDELAY (IDELAY, ODELAY) statement to a
signal, the last statement overrules the previous statements, and HSPICE
or HSPICE RF issues a warning.
■
If you do not specify the signal delays in a TDELAY, IDELAY, or ODELAY
statement, HSPICE or HSPICE RF defaults to zero.
See Also
IDELAY
TDELAY
TUNIT
HSPICE® Command Reference
X-2005.09
399
4: Commands in Digital Vector Files
OUT or OUTZ
OUT or OUTZ
Syntax
OUT <output_resistance> mask
Argument
Definition
<output_resistance>
Output resistance for an input signal. Default=0.
mask
Signals to which the output resistance applies. If you do not
provide a mask, the output resistance value applies to all input
signals.
Example
OUT 15.1
OUT 150 1 1 1 0000 00000000
OUTZ 50.5 0 0 0 137F 00000000
The first OUT statement in this example creates a 15.1 ohm resistor to place in
series with all vector inputs. The next OUT statement sets the resistance to 150
ohms for vectors 1 to 3. The OUTZ statement changes the resistance to 50.5
ohms for vectors 4 through 7.
Description
The OUT and OUTZ keywords are equivalent, and specify output resistance for
each signal (for which the mask applies); OUT (or OUTZ) applies only to input
signals.
■
If you do not specify the output resistance of a signal in an OUT (or OUTZ)
statement, HSPICE or HSPICE RF uses the default (zero).
■
If you specify more than one OUT (or OUTZ) statement for a signal, the last
statement overrules the previous statements, and HSPICE or HSPICE RF
issues a warning message.
The OUT (or OUTZ) statements have no effect on the expected output signals.
400
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
PERIOD
PERIOD
Syntax
PERIOD time_interval
Argument
Definition
time_interval
Time interval for the Tabular Data.
Example
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.
Description
The PERIOD statement defines 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 statement without the TSKIP statement, the Tabular Data section
contains only signal values, not absolute times. The TUNIT statement defines
the time unit of the PERIOD.
HSPICE® Command Reference
X-2005.09
401
4: Commands in Digital Vector Files
RADIX
RADIX
Syntax
RADIX <number_of_bits> [<number_of_bits>...]
Argument
Definition
<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 statement for each vector listed in the file.
Example
; 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.
Description
The RADIX statement specifies the number of bits associated with each vector.
Valid values for the number of bits range from 1 to 4.
Table 1 Valid Values for the RADIX Statement
# 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
A digital vector file must contain only one RADIX command, and it must be the
first non-comment line in the file.
402
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
SLOPE
SLOPE
Syntax
SLOPE [<input_rise_time> | <input_fall_time>] mask
Argument
Definition
<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 statement applies. If you
do not specify a mask, the SLOPE statement applies to all
signals.
Example 1
SLOPE 1.2
In this example, the rising and falling times of all signals are 1.2 ns.
Example 2
SLOPE 1.1 1100 0110
In this example, the rising/falling time is 1.1 ns for the first, second, sixth, and
seventh signals.
Description
The SLOPE statement specifies the rise/fall time for the input signal. Use the
TUNIT statement to define the time unit for this statement.
■
If you do not specify the SLOPE statement, the default slope value is 0.1 ns.
■
If you specify more than one SLOPE statement, the last statement overrules
the previous statements, and HSPICE or HSPICE RF issues a warning
message.
The SLOPE statement has no effect on the expected output signals. You can
specify the optional TRISE and TFALL statements to overrule the rise time and
fall time of a signal.
HSPICE® Command Reference
X-2005.09
403
4: Commands in Digital Vector Files
TDELAY
TDELAY
Syntax
TDELAY delay_value mask
Argument
Definition
delay_value
Time delay to apply to the signals.
mask
Signals to which the delay applies. If you do not provide a mask,
the delay value applies to all signals.
Example
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 statement so HSPICE or HSPICE
RF uses the default, ns, as the time unit for this example. The first TDELAY
statement indicates that all signals have the same delay time of 1.0ns.
Subsequent TDELAY, IDELAY, or ODELAY statements 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.
Description
Defines 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 statement.
404
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
TDELAY
■
If you apply more than one TDELAY (IDELAY, ODELAY) statement to a
signal, the last statement overrules the previous statements, and HSPICE
or HSPICE RF issues a warning.
■
If you do not specify the signal delays in a TDELAY, IDELAY, or ODELAY
statement, HSPICE or HSPICE RF defaults to zero.
See Also
IDELAY
ODELAY
TUNIT
HSPICE® Command Reference
X-2005.09
405
4: Commands in Digital Vector Files
TFALL
TFALL
Syntax
TFALL <input_fall_time> mask
Argument
Definition
<input_fall_time>
Fall time of the input signal.
mask
Name of a signal to which the TFALL statement applies. If you
do not specify a mask, the TFALL statement applies to all input
signals.
Example
In the following example, the TFALL statement assigns a fall time of 0.5 time
units to all vectors.
TFALL 0.5
In the following example, the TFALL statement assigns a fall time of 0.3 time
units, overriding the older setting of 0.5 to vectors 2, 3, and 4 to 7.
TFALL 0.3 0 1 1 137F 00000000
In the following example, the TFALL statement assigns a fall time of 0.9 time
units to vectors 8 through 11.
TFALL 0.9 0 0 0 0000 11110000
Description
The TFALL statement specifies the fall time of each input signal for which the
mask applies. The TUNIT statement defines the time unit of TFALL.
■
If you do not use any TFALL statement to specify the fall time of the signals,
HSPICE or HSPICE RF uses the value defined in the slope statement.
■
If you apply more than one TFALL statement to a signal, the last statement
overrules the previous statements, and HSPICE or HSPICE RF issues a
warning message.
TFALL statements have no effect on the expected output signals.
406
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
TRISE
TRISE
Syntax
TRISE <input_rise_time> mask
Argument
Definition
<input_rise_time>
Rise time of the input signal.
mask
Name of a signal to which the TRISE statement applies. If you
do not specify a mask, the TRISE statement applies to all input
signals.
Example 1
TRISE 0.3
In this example, the TRISE statement assigns a rise time of 0.3 time units to all
vectors.
Example 2
TRISE 0.5 0 1 1 137F 00000000
In this example, the TRISE statement 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 3
TRISE 0.8 0 0 0 0000 11110000
In this example, the TRISE statement assigns a rise time of 0.8 time units to
vectors 8 through 11.
Description
The TRISE statement specifies the rise time of each input signal for which the
mask applies. The TUNIT statement defines the time unit of TRISE.
■
If you do not use any TRISE statement to specify the rising time of the
signals, HSPICE or HSPICE RF uses the value defined in the slope
statement.
HSPICE® Command Reference
X-2005.09
407
4: Commands in Digital Vector Files
TRISE
■
If you apply more than one TRISE statement to a signal, the last statement
overrules the previous statements, and HSPICE or HSPICE RF issues a
warning message.
TRISE statements have no effect on the expected output signals.
408
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
TRIZ
TRIZ
Syntax
TRIZ <output_impedance>
Argument
Definition
<output_impedance>
Output impedance of the input signal.
mask
Name of a signal to which the TRIZ statement applies. If
you do not specify a mask, the TRIZ statement applies to
all input signals.
Example
TRIZ 15.1Meg
TRIZ 150Meg 1 1 1 0000 00000000
TRIZ 50.5Meg 0 0 0 137F 00000000
■
The first TRIZ statement sets the high impedance resistance globally, at
15.1 Mohms.
■
The second TRIZ statement increases the value to 150 Mohms, for vectors
1 to 3.
■
The last TRIZ statement increases the value to 50.5 Mohms, for vectors 4
through 7.
Description
The TRIZ statement specifies 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 statement,
HSPICE or HSPICE RF assumes 1000M.
■
If you apply more than one TRIZ statement to a signal, the last statement
overrules the previous statements, and HSPICE or HSPICE RF issues a
warning.
TRIZ statements have no effect on the expected output signals.
HSPICE® Command Reference
X-2005.09
409
4: Commands in Digital Vector Files
TSKIP
TSKIP
Syntax
TSKIP <absolute_time> <tabular_data> ...
Argument
Definition
<absolute_time>
Absolute time.
<tabular_data>
Data captured at <absolute_time>.
Example
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.
Description
The TSKIP statement specifies to ignore the absolute time field in the tabular
data. You can then keep, but ignore, the absolute time field of each row in the
tabular data, when you use the PERIOD statement.
You might do this, for example, if the absolute times are not perfectly periodic
for testing reasons. 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 or
HSPICE RF writes to the vector file, using absolute time. After you fix the
circuit, you might want to use periodic data.
410
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
TUNIT
TUNIT
TUNIT [fs|ps|ns|us|ms]
Argument
Definition
fs
femtosecond
ps
picosecond
ns
nanosecond (this is the default)
us
microsecond
ms
millisecond
Example
TUNIT ns
11.0 1000 1000
20.0 1100 1100
33.0 1010 1001
The TUNIT statement in this example specifies that the absolute times in the
Tabular Data section are 11.0ns, 20.0ns, and 33.0ns.
Description
The TUNIT statement defines 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 statement, the default time unit value is ns.
■
If you define more than one TUNIT statement, the last statement overrules
the previous statement.
See Also
IDELAY
ODELAY
TDELAY
HSPICE® Command Reference
X-2005.09
411
4: Commands in Digital Vector Files
VIH
VIH
Syntax
VIH <logic-high_voltage> mask
Argument
Definition
<logic-high_voltage>
Logic-high voltage for an input signal. Default=3.3.
mask
Name of a signal to which the VIH statement applies. If you
do not specify a mask, the VIH statement applies to all input
signals.
Example
VIH 5.0
VIH 3.5 0 0 0 0000 11111111
■
The first VIH statement sets all input vectors to 5V, when they are high.
■
The last VIH statement changes the logic-high voltage from 5V to 3.5V, for
the last eight vectors.
Description
The VIH statement specifies 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 statement,
HSPICE or HSPICE RF assumes 3.3.
■
If you use more than one VIH statement for a signal, the last statement overrules previous statements. HSPICE or HSPICE RF issues a warning.
VIH statements have no effect on the expected output signals.
See Also
VIL
VOH
VOL
VTH
412
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
VIL
VIL
Syntax
VIL <logic-low_voltage>
Argument
Definition
<logic-low_voltage>
Logic-low voltage for an input signal. Default=0.0.
mask
Name of a signal to which the VIL statement applies. If you
do not specify a mask, the VIL statement applies to all input
signals.
Example
VIL 0.0
VIL 0.5 0 0 0 0000 11111111
■
The first VIL statement sets the logic-low voltage to 0V, for all vectors.
■
The second VIL statement changes the logic-low voltage to 0.5V, for the last
eight vectors.
Description
The VILstatement specifies 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 statement,
HSPICE or HSPICE RF assumes 0.0.
■
If you use more than one VIL statement for a signal, the last statement overrules previous statements. HSPICE or HSPICE RF issues a warning.
VIL statements have no effect on the expected output signals.
See Also
VIH
VOH
VOL
VTH
HSPICE® Command Reference
X-2005.09
413
4: Commands in Digital Vector Files
VNAME
VNAME
Syntax
VNAME vector_name[[starting_index : ending_index]]
Argument
Definition
<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
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
VNAME a[[0:3]]
This example 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]]. The high bit is a4, which represents 24. It is the largest
value, and therefore is the MSB.
Example 3
RADIX 2 4
VNAME VA[[0:1]] VB[[4:1]]
414
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
VNAME
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 4
VNAME VA[[0:1]] VB<[4:1]>
HSPICE or HSPICE RF generates voltage sources with the following names:
VA[0] VA[1] VB<4> VB<3> VB<2> VB<1>
Example 5
VNAME VA[[2:2]]
This example specifies a single bit of a bus. This range creates a voltage
source named:
VA[2]
Example 6
RADIX 444444
VNAME A[[0:23]]
This example generates signals named A0, A1, A2, ... A23.
Description
The VNAME statement defines 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 statement, the last
statement overrules the previous statement.
HSPICE® Command Reference
X-2005.09
415
4: Commands in Digital Vector Files
VOH
VOH
Syntax
VOH <logic-high_voltage> mask
Argument
Definition
<logic-high_voltage>
Logic-high voltage for an output vector. Default=2.66.
mask
Name of a signal to which the VOH statement applies. If
you do not specify a mask, the VOH statement applies
to all output signals.
Example
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 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 output.
These second and third lines completely override the first VOH statement.
If you do not define either VOH or VOL, HSPICE or HSPICE RF uses VTH
(default or defined).
Description
The VOH statement specifies the logic-high voltage, for each output signal to
which the mask applies.
■
If you do not specify the logic-high voltage in a VOH statement, HSPICE or
HSPICE RF assumes 2.64.
■
If you apply more than one VOH statement to a signal, the last statement
overrules the previous statements, and HSPICE or HSPICE RF issues a
warning.
VOH statements have no effect on input signals.
416
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
VOH
See Also
VIH
VIL
VOL
VTH
HSPICE® Command Reference
X-2005.09
417
4: Commands in Digital Vector Files
VOL
VOL
Syntax
VOL <logic-low_voltage> mask
Argument
Definition
<logic-low_voltage>
Logic-low voltage for an output vector. Default=0.64.
mask
Name of a signal to which the VOL statement applies. If
you do not specify a mask, the VOL statement applies
to all output signals.
Example
VOL 0.0
VOL 0.2 0 0 0 137F 00000000
VOL 0.5 1 1 1 0000 00000000
■
The first VOL statement sets the logic-low output to 0V.
■
The second VOL statement sets the output voltage to 0.2V, for the fourth
through seventh vectors.
■
The last statement increases the voltage further to 0.5V, for the first three
vectors.
These second and third lines completely override the first VOL statement.
If you do not define either VOH or VOL, HSPICE or HSPICE RF uses VTH
(default or defined).
Description
The VOL statement specifies the logic-low voltage, for each output signal to
which the mask applies.
418
■
If you do not specify the logic-low voltage, in a VOL statement, HSPICE or
HSPICE RF assumes 0.66.
■
If you apply more than one VOL statement to a signal, the last statement
overrules the previous statements, and HSPICE or HSPICE RF issues a
warning.
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
VOL
See Also
VIH
VIL
VOH
VTH
HSPICE® Command Reference
X-2005.09
419
4: Commands in Digital Vector Files
VREF
VREF
Syntax
VREF <reference_voltage>
Argument
Definition
<reference_voltage>
Reference voltage for each input vector. Default=0.
Example
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 statements 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.
Description
Similar to the TDELAY statement, the VREF statement specifies the name of the
reference voltage, for each input vector to which the mask applies. VREF
applies only to input signals.
■
If you do not specify the reference voltage name of the signals, in a VREF
statement, HSPICE or HSPICE RF assumes 0.
■
If you apply more than one VREF statement, the last statement overrules the
previous statements, and HSPICE or HSPICE RF issues a warning.
VREF statements have no effect on the output signals.
420
HSPICE® Command Reference
X-2005.09
4: Commands in Digital Vector Files
VTH
VTH
Syntax
VTH <logic-threshold_voltage>
Argument
Definition
<logic-threshold_voltage>
Logic-threshold voltage for an output vector.
Default=1.65.
Example
VTH 1.75
VTH 2.5 1 1 1 137F 00000000
VTH 1.75 0 0 0 0000 11111111
■
The first VTH statement 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 statements, so the vectors are all bidirectional.
Description
Similar to the TDELAY statement, the VTH statement specifies the logic
threshold voltage, for each output signal to which the mask applies. 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 statement,
HSPICE or HSPICE RF assumes 1.65.
■
If you apply more than one VTH statement to a signal, the last statement
overrules the previous statements, and HSPICE or HSPICE RF issues a
warning.
VTH statements have no effect on the input signals.
HSPICE® Command Reference
X-2005.09
421
4: Commands in Digital Vector Files
VTH
See Also
VIH
VIL
VOH
VOL
422
HSPICE® Command Reference
X-2005.09
Index
A
ABSH option 195
ABSI option 196, 286
ABSMOS option 197, 286
ABSTOL option 198
ABSV option 199
ABSVAR option 200
ABSVDC option 201
AC analysis
magnitude 204
optimization 9
output 204
phase 204
.AC command 9
external data 29
ACCURATE option 203
ACOUT option 204
algorithms
DVDT 200, 292
local truncation error 292, 342, 368
pivoting 325
timestep control 254
transient analysis timestep 292
trapezoidal integration 303
.ALIAS command 14
ALL keyword 134, 158
ALT9999 option 205
ALTCC option 206
ALTCHK option 207
alter block commands 1
.ALTER command 16, 44
Analog Artist interface 336
See also Artist
Analysis commands 1
analysis, network 129
arithmetic expression 111
HSPICE® Command Reference
X-2005.09
ARTIST option 208, 336
ASCII output data 221, 301, 355
ASPEC option 209
AT keyword 109
autoconvergence 238
AUTOSTOP option 210
average measurements, with .MEASURE 105
average nodal voltage, with .MEASURE 112
average value, measuring 112
AVG keyword 113
B
BADCHR option 211, 212
BETA keyword 156
.BIASCHK command 18
BIASFILE option 213
BIAWARN option 214
BINPRINT option 215
bisection
pushout 121
BKPSIZ option 216
branch current error 196
breakpoint table, size 216
BRIEF option 134, 135, 217, 291, 309, 318, 322
BSIM model, LEVEL 13 128
BSIM2 model, LEVEL 39 128
bus notation 414
BYPASS option 218
BYTOL option 219
C
Cadence
Opus 221, 355
WSF format 221, 355
423
Index
C
capacitance
charge tolerance, setting 222
CSHUNT node-to-ground 229
table of values 220
capacitor, models 124
CAPTAB option 220
CDS option 221
CENDIF optimization parameter 125
characterization of models 35
charge tolerance, setting 222
CHGTOL option 222
CLOSE optimization parameter 125
CMIFLAG option 223
CO option 181, 186, 224
column laminated data 28
commands
.AC 9
.ALIAS 14
.ALTER 16, 44
alter block 1
analysis 1
.BIASCHK 18
.CONNECT 23
.DATA 25
.DC 32
.DCMATCH 38
.DCVOLT 40
.DEL LIB 42
.DISTO 46
.DOUT 49
.EBD 52
.ELSE 54
.ELSEIF 55
.END 56
.ENDDATA 57
.ENDIF 58
.ENDL 59
.ENDS 60
.EOM 61
.FFT 62
.FOUR 65
.FSOPTIONS 66
.GLOBAL 68
.GRAPH 69
.HDL 71
.IBIS 72
.IC 76
.ICM 78
424
.IF 79
.INCLUDE 81
.LAYERSTACK 82
.LIB 84
.LOAD 91
.MACRO 93
.MALIAS 96
.MATERIAL 98
.MEASURE 100
.MODEL 123
.NET 129
.NODESET 131
.NOISE 132
.OP 133
.PARAM 137
.PAT 141
.PKG 143
.PLOT 145
.PRINT 147
.PROBE 151
.PROTECT 153
.PZ 154
.SAVE 157
.SENS 159
.SHAPE 161
.STIM 167
subcircuit 5
.SUBCKT 172
.TEMP 175
.TF 177
.TITLE 178
.TRAN 179
.UNPROTECT 184
.VEC 185
Verilog-A 5
.WIDTH 186
Common Simulation Data Format 252
concatenated data files 27
Conditional Block 2
conductance
current source, initialization 265
minimum, setting 266
models 239
MOSFETs 267
negative, logging 251
node-to-ground 270
sweeping 268
.CONNECT command 23
HSPICE® Command Reference
X-2005.09
Index
D
control options
printing 322
setting 135
transient analysis
limit 372
CONVERGE option 225, 240
convergence
for optimization 127
problems
causes 218
changing integration algorithm 303
CONVERGE option 225, 240
DCON setting 238
decreasing the timestep 261
.NODESET statement 131
nonconvergent node listing 238
operating point Debug mode 134
setting DCON 238
steady state 268
CPTIME option 226
CPU time, reducing 310
CROSS keyword 108
CSDF option 227
CSHDC option 228
CSHUNT option 229
current
ABSMOS floor value for convergence 341
branch 196
operating point table 134
CURRENT keyword 134
CUSTCMI option 230
CUT optimization parameter 125
CVTOL option 231
D
D_IBIS option 232
.DATA command 25, 26
datanames 29
external file 25
for sweep data 29
inline data 29
data files, disabling printout 217, 318
DATA keyword 11, 28, 35, 181
datanames 29, 169
DC
analysis
decade variation 36
HSPICE® Command Reference
X-2005.09
initialization 236
iteration limit 278
linear variation 36
list of points 36
octave variation 36
optimization 32
.DC command 32, 35
external data with .DATA 29
DCAP option 233
DCCAP option 234
DCFOR option 235
DCHOLD option 236
DCIC option 237
.DCMATCH command 38
DCON option 238
DCSTEP option 239
DCTRAN option 240
.DCVOLT command 40, 76
DEBUG keyword 134
DEC keyword 12, 36, 182
DEFAD option 241
DEFAS option 242
DEFL option 243
DEFNRD option 244
DEFNRS option 245
DEFPD option 246
DEFPS option 247
DEFW option 248
.DEL LIB command 42
with .ALTER 44
with .LIB 44
delays
group 369
DELMAX option 249, 349
DELTA internal timestep 249
See also timestep
derivative function 116
DERIVATIVE keyword 117
derivatives, measuring 108
DI option 250
DIAGNOSTIC option 251
DIFSIZ optimization parameters 126
DIM2 distortion measure 47
DIM3 distortion measure 47
diode models 124
.DISTO command 46
425
Index
E
distortion
HD2 47
HD3 48
distortion measures
DIM2 47
DIM3 47
DLENCSDF option 252
.DOUT command 49
DV option 238, 253
DVDT
algorithm 200, 345
option 254, 292
DVDT option 254
DVTR option 255
E
.EBD command 52
element
checking, suppression of 310
OFF parameter 319
.ELSE command 54
.ELSE statement 54
.ELSEIF command 55
Encryption 2
.END command 56
for multiple HSPICE runs 56
location 56
.ENDDATA command 57
ENDDATA keyword 25, 27, 30
.ENDIF command 58
.ENDL command 59, 86
.ENDS command 60
.EOM command 61
EPSMIN option 256
equation 111
ERR function 119
ERR1 function 119
ERR2 function 119
ERR3 function 119
error function 119
errors
branch current 196
function 119
internal timestep too small 229, 350
optimization goal 103
tolerances
426
ABSMOS 197
branch current 196
RELMOS 197
voltage 343, 344, 346
example, subcircuit test 93, 172
EXPLI option 257
EXPMAX option 258
expression, arithmetic 111
external data files 30
F
FALL keyword 108
FAST option 259
.FFT command 62
FFTOUT option 260
FIL keyword 30
files
column lamination 28
concatenated data files 27
filenames 30
hspice.ini 301
include files 81, 85
multiple simulation runs 56
FIND keyword 108
FIND, using with .MEASURE 107
floating point overflow
CONVERGE setting 225
setting GMINDC 267
.FOUR command 65
frequency
ratio 47
sweep 10
FROM parameter 120
FS option 156, 261
.FSOPTIONS command 66
FT option 262
functions
ERR 119
ERR1 119
ERR2 119
ERR3 119
error 119
G
GDCPATH option 263
GENK option 264
HSPICE® Command Reference
X-2005.09
Index
H
.GLOBAL command 68
global node names 68
GMAX option 265
GMIN option 266, 267
GMINDC option 267
GOAL keyword 113
GRAD optimization parameter 126
GRAMP
calculation 238
option 268
.GRAPH command 69
graph data file (Viewlogic format) 252
group delay, calculating 369
GSHDC option 269
GSHUNT option 270
H
H9007 option 271
harmonic distortion 47
HD2 distortion 47
HD3 distortion 48
.HDL command 71
HIER_SCALE option 272
HSPICE
job statistics report ??–202
version
H9007 compatibility 271
parameter 128
hspice.ini file 301
I
.IBIS command 72
IBIS commands 3
.IC command 40, 76
from .SAVE 157
IC parameter 40, 76, 157
.ICM command 78
ICSWEEP option 273
.IF command 79
IGNOR keyword 119
IMAX option 274, 281
IMIN option 275, 280
.INCLUDE command 81
include files 81, 85
indepout 169
HSPICE® Command Reference
X-2005.09
indepvar 169, 170
inductors, mutual model 124
INGOLD option 276, 297
initial conditions
saving and reusing 273
transient 182
initialization 319
inline data 29
inner sweep 26
input
data
adding library data 44
column laminated 28
concatenated data files 27
deleting library data 44
external, with .DATA statement 29
filenames on networks 28
formats 28, 29
include files 81
printing 291
suppressing printout 291
netlist file 56
INTEG keyword 113, 115
used with .MEASURE 112
integral function 115
integration
backward Euler method 294
order of 294
interfaces
Analog Artist 336
Mentor 302
MSPICE 302
ZUKEN 379
intermodulation distortion 47
INTERP option 277
iterations
limit 278
maximum number of 282
ITL1 option 278
ITL2 option 279
ITL3 option 280
ITL4 option 281
ITL5 option 282
ITLPTRAN option 283
ITLPZ option 284
ITROPT optimization parameter 126
ITRPRT option 285
427
Index
J
J
Jacobian data, printing 321
K
KCLTEST option 286
keywords
.AC statement parameter 11
ALL 134, 158
AT 109
AVG 113
BETA 156
CROSS 108
CURRENT 134
DATA 11, 28, 35, 181
.DATA command parameter 28
.DC command parameter 35
DEBUG 134
DEC 12, 36, 182
DERIVATIVE 117
ENDDATA 25, 27, 30
FALL 108
FIL 30
FIND 108
FS 156
IGNOR 119
INTEG 112, 113, 115
LAM 28, 30
LAST 109
LIN 12, 36, 182
MAXFLD 156
.MEASUREMENT command parameter 113
MER 27, 28, 30
MINVAL 120
MODEL 35
.MODEL statement parameters 123
MONTE 12, 181
NONE 134, 158
NUMF 156
OCT 12, 36, 182
OPTIMIZE 35
PLOT 123
POI 12, 36, 182
PP 112, 113
RESULTS 35
RIN 130
RISE 108
START 182
428
SWEEP 12, 36, 182
target syntax 109
TO 113, 120
TOL 156
TOP 158
.TRAN command parameter 181
TRIG 101
VOLTAGE 134
WEIGHT 113, 120
weight 113
WHEN 108
Kirchhoff’s Current Law (KCL) test 286
KLIM option 287
L
LAM keyword 28, 30
laminated data 28
LAST keyword 109
latent devices
BYPASS option 218
excluding 259
.LAYERSTACK command 82
LENNAM option 288
LEVEL 13 BSIM model 128
LEVEL parameter 126
.LIB command 84
call statement 86
in .ALTER blocks 86
nesting 86
with .DEL LIB 44
libraries
adding with .LIB 44
building 86
DDL 356
defining macros 86
deleting 42
private 153
protecting 153
Library Management 3
LIMPTS option 289
LIMTIM option 290
LIN keyword 12, 36, 182
LIST option 291
listing, suppressing 153
.LOAD command 91
local truncation error algorithm 292, 342, 368
HSPICE® Command Reference
X-2005.09
Index
M
LVLTIM option 292, 303, 345, 368
M
.MACRO command 93
macros 44, 86
magnetic core models 124
.MALIAS command 96
.MATERIAL command 98
Material Properties 3
matrix
minimum pivot values 329
parameters 129
row/matrix ratio 328
size limitation 327
MAX 112
MAX parameter 113, 126
MAXAMP option 293
MAXFLD keyword 156
maximum value, measuring 112
MAXORD option 294
MBYPASS option 295
MCBRIEF option 296
MEASDGT option 297
MEASFAIL option 298
MEASFILE option 299
MEASOUT option 301
MEASSORT option 300
.MEASURE command 100, 297, 301
average measurements 105
average nodal voltage 112
expression 111
propogation delay 101
measuring average values 112
measuring derivatives 108
Mentor interface 302
MENTOR option 302
MER keyword 27, 28, 30
messages
See also errors, warnings
messages, pivot change 326
METHOD option 303
MIN 112
MIN parameter 113
minimum value, measuring 112
MINVAL keyword 120
HSPICE® Command Reference
X-2005.09
.MODEL command 123
CENDIF 125
CLOSE 125
CUT 125
DEV 125
DIFSIZ 126
distribution 126
GRAD 126
HSPICE version parameter 128
ITROPT 126
keyword 126
LEVEL 126
LOT 126
MAX 126
model name 124
PARMIN 127
PLOT 127
RELIN 127
RELOUT 127
type 124
VERSION 128
MODEL keyword 35
model parameters
LEVEL 126
suppressing printout of 312
TEMP 176
models
BJTs 124
BSIM LEVEL 13 128
BSIM2 LEVEL 39 128
capacitors 124
characterization 35
diode 124
JFETs 124
magnetic core 124
MOSFETs 124
mutual inductors 124
names 124
npn BJT 124
op-amps 124
optimization 124
plot 124
private 153
protecting 153
simulator access 86
types 124
models, diode 124
MODMONTE option 304
429
Index
N
MODSRH option 305
Monte Carlo
AC analysis 10
DC analysis 32
.MODEL parameters 126
time analysis 180
MONTE keyword 12, 181
MONTECON option 306
MSPICE simulator interface 302
MU option 307
N
namei 168, 169, 170
n-channel, MOSFET’s models 124
negative conductance, logging 251
nested library calls 86
.NET comamnd 129
network
analysis 129
filenames 28
network analysis 129
NEWTOL option 308
Node Naming 4
NODE option 309
nodes
cross-reference table 309
global versus local 68
printing 309
.NODESET command 131, 235
DC operating point initialization 131
from .SAVE 157
NODESET keyword 157
node-to-element list 326
NOELCK option 310
noise
folding 156
numerical 229
sampling 156
.NOISE command 132
NOISEMINFREQ option 311
NOMOD option 312
NONE keyword 134, 158
NOPAGE option 313
NOPIV option 314
NOTOP option 315
NOWARN option 316
430
npn BJT models 124
npoints 168, 169, 170
NUMDGT option 317
numerical integration algorithms 303
numerical noise 229, 270
NUMF keyword 156
NXX option 318
O
OCT keyword 12, 36, 182
OFF option 319
.OP command 133
op-amps model, names 124
operating point
capacitance 220
.IC statement initialization 40, 76
.NODESET statement initialization 131
restoring 92
solution 319
voltage table 134
OPFILE option 320
optimization
AC analysis 9
algorithm 126
DC analysis 32
error function 103
iterations 126
models 124
time
analysis 180
required 125
optimization parameter, DIFSIZ 126
OPTIMIZE keyword 35
.OPTION 135
SEARCH 356
.OPTION ABSH 195
.OPTION ABSI 196
.OPTION ABSMOS 197
.OPTION ABSTOL 198
.OPTION ABSV 199
.OPTION ABSVAR 200
.OPTION ABSVDC 201
.OPTION ACCT 201
.OPTION ACCURATE 203
.OPTION ACOUT 204
.OPTION ALT999 203
HSPICE® Command Reference
X-2005.09
Index
O
.OPTION ALT9999 205
.OPTION ALTCC 206
.OPTION ALTCHK 207
.OPTION ARTIST 208, 336
.OPTION ASPEC 209
.OPTION AUTOSTOP 210
.OPTION BADCHR 211, 212
.OPTION BIASFILE 213
.OPTION BIAWARN 214
.OPTION BINPRINT 215
.OPTION BKPSIZ 216
.OPTION BRIEF 134, 135, 217, 291, 309, 318,
322
.OPTION BYPASS 218
.OPTION BYTOL 219
.OPTION CAPTAB 220
.OPTION CDS 221
.OPTION CHGTOL 222
.OPTION CMIFLAG 223
.OPTION CO 181, 186, 224
.OPTION CONVERGE 225
.OPTION CPTIME 226
.OPTION CSDF 227
.OPTION CSHDC 228
.OPTION CSHUNT 229
.OPTION CUSTCMI 230
.OPTION CVTOL 231
.OPTION D_IBIS 232
.OPTION DCAP 233
.OPTION DCCAP 234
.OPTION DCFOR 235
.OPTION DCHOLD 236
.OPTION DCIC 237
.OPTION DCON 238
.OPTION DCSTEP 239
.OPTION DCTRAN 240
.OPTION DEFAD 241
.OPTION DEFAS 242
.OPTION DEFL 243
.OPTION DEFNRD 244
.OPTION DEFNRS 245
.OPTION DEFPD 246
.OPTION DEFPS 247
.OPTION DEFW 248
.OPTION DELMAX 249
HSPICE® Command Reference
X-2005.09
.OPTION DI 250
.OPTION DIAGNOSTIC 251
.OPTION DLENCSDF 252
.OPTION DV 253
.OPTION DVDT 254
.OPTION DVTR 255
.OPTION EPSMIN 256
.OPTION EXPLI 257
.OPTION EXPMAX 258
.OPTION FAST 259
.OPTION FFTOUT 260
.OPTION FS 261
.OPTION FT 262
.OPTION GDCPATH 263
.OPTION GENK 264
.OPTION GMAX 265
.OPTION GMIN 266
.OPTION GMINDC 267
.OPTION GRAMP 268
.OPTION GSHDC 269
.OPTION GSHUNT 270
.OPTION H9007 271
.OPTION HIER_SCALE 272
.OPTION ICSWEEP 273
.OPTION IMAX 274
.OPTION IMIN 275
.OPTION INGOLD 276
.OPTION INTERP 277
.OPTION ITL1 278
.OPTION ITL2 279
.OPTION ITL3 280
.OPTION ITL4 281
.OPTION ITL5 282
.OPTION ITLPTRAN 283
.OPTION ITLPZ 284
.OPTION ITRPRT 285
.OPTION KCLTEST 286
.OPTION KLIM 287
.OPTION LENNAM 288
.OPTION LIMPTS 289
.OPTION LIMTIM 290
.OPTION LIST 291
.OPTION LVLTIM 292
.OPTION MAXAMP 293
.OPTION MAXORD 294
431
Index
O
.OPTION MBYPASS 295
.OPTION MCBRIEF 296
.OPTION MEASDGT 297
.OPTION MEASFAIL 298
.OPTION MEASFILE 299
.OPTION MEASOUT 301
.OPTION MEASSORT 300
.OPTION MENTOR 302
.OPTION METHOD 303
.OPTION MODMONTE 304
.OPTION MODSRH 305
.OPTION MONTECON 306
.OPTION MU 307
.OPTION NEWTOL 308
.OPTION NODE 309
.OPTION NOELCK 310
.OPTION NOISEMINFREQ 311
.OPTION NOMOD 312
.OPTION NOPAGE 313
.OPTION NOPIV 314
.OPTION NOTOP 315
.OPTION NOWARN 316
.OPTION NUMDGT 317
.OPTION NXX 318
.OPTION OFF 319
.OPTION OPFILE 320
.OPTION OPTLST 321
.OPTION OPTS 322
.OPTION PARHIER 323
.OPTION PATHNUM 324
.OPTION PIVOT 325
.OPTION PIVREF 327
.OPTION PIVREL 328
.OPTION PIVTOL 329
.OPTION PLIM 330
.OPTION POST 331
.OPTION POST_VERSION 333
.OPTION POSTTOP 334
.OPTION PROBE 335
.OPTION PSF 336
.OPTION PURETP 337
.OPTION PUTMEAS 338
.OPTION RELH 339
.OPTION RELI 340
.OPTION RELMOS 341
432
.OPTION RELQ 342
.OPTION RELTOL 343
.OPTION RELV 344
.OPTION RELVAR 345
.OPTION RELVDC 346
.OPTION RESMIN 347
.OPTION RMAX 349
.OPTION RMIN 350
.OPTION RUNLVL 351
.OPTION SCALE 353
.OPTION SCALM 354
.OPTION SDA 355
.OPTION SEARCH 356
.OPTION SEED 357
.OPTION SLOPETOL 358
.OPTION SPARSE 359
.OPTION SPICE 360
.OPTION SPMODEL 361
.OPTION STATFL 362
.OPTION SYMB 363
.OPTION TIMERES 364
.OPTION TNOM 365
.OPTION TRCON 366
.OPTION TRTOL 368
.OPTION UNWRAP 369
.OPTION VAMODEL 370
.OPTION VERIFY 371
.OPTION VFLOOR 372
.OPTION VNTOL 373
.OPTION WACC 374
.OPTION WARNLIMIT 376
.OPTION WL 377
.OPTION WNFLAG 375
.OPTION XDTEMP 378
.OPTION ZUKEN 379
OPTLST option 321
OPTS option 322
Opus 221, 355
oscillation, eliminating 303
outer sweep 26
Output 4
output
data
format 297, 336
limiting 277
HSPICE® Command Reference
X-2005.09
Index
P
significant digits specification 317
specifying 289
storing 301
files
reducing size of 376
.MEASURE results 100
plotting 145
printing 147–150
printout format 276
variables
printing 285
probing 151
specifying significant digits for 317
ovari 168, 170
P
.PARAM command 137
parameters
AC sweep 9
DC sweep 32
defaults 323
FROM 120
IC 40, 76
inheritance 323
ITROPT optimization 126
LEVEL 126
matrix 129
names
.MODEL command
parameter name 127
simulator access 86
skew, assigning 85
UIC 40, 76
PARHIER option 323
PARMIN optimization parameter 127
.PAT command 141
path names 324
path numbers, printing 324
PATHNUM option 324
p-channel
JFETs models 124
MOSFET’s models 124
Peak 105
peak measurement 105
peak-to-peak value 115
measuring 112
PERIOD statement 401, 411
HSPICE® Command Reference
X-2005.09
pivot
algorithm, selecting 325
change message 326
reference 327
PIVOT option 325
PIVREF option 327
PIVREL option 328
PIVTOL option 325, 329
.PKG command 143
PLIM option 330
plot
models 124
value calculation method 204
.PLOT command 145
in .ALTER block 16
PLOT keyword 123
pnp BJT models 124
POI keyword 12, 36, 182
pole/zero analysis, maximum iterations 284
polygon, defining 166
POST_VERSION option 333
POSTTOP option 334
power operating point table 134
PP 112, 115
PP keyword 112, 113
.PRINT command 147
in .ALTER 16
printing
Jacobian data 321
printout
disabling 217, 318
suppressing 153
value calculation method 204
.PROBE command 151
PROBE option 335
propogation delays
measuring 102
with .MEASURE 101
.PROTECT command 153
protecting data 153
PSF option 336
PURETP option 337
pushout bisection 121
PUTMEAS option 338
.PZ command 154
433
Index
R
R
reference temperature 176
RELH option 339
RELI option 286, 340
RELIN optimization parameter 127
RELMOS option 197, 286, 341
RELOUT optimization parameter 127
RELQ option 342
RELTOL option 222, 343
RELTOLoption 343
RELV option 259, 295, 344
RELVAR option 345
RELVDC option 344, 346
resistance 347
RESMIN option 347
RESULTS keyword 35
RIN keyword 130
Rise 101
rise and fall times 102
RISE keyword 108
rise time
specify 406, 407
RISETIME option 348
RMAX option 349
RMIN option 350
RMS
measurement 105
used with .MEASURE 105
RMS keyword 113
ROUT keyword 130
row/matrix ratio 328
RUNLVL option 351
S
S parameter, model type 124
.SAMPLE 156
.SAMPLE statement 156
sampling noise 156
.SAVE command 157
SCALE option 353
SCALM option 354
Schmitt trigger example 34
SDA option 355
SEARCH option 356
434
SEED option 357
.SENS command 159
Setup 4
.SHAPE command 161
Defining Circles 163
Defining Polygons 164
Defining Rectangles 162
Defining Strip Polygons 166
SIM2 distortion measure 48
simulation
accuracy 203, 292
improvement 254
multiple analyses, .ALTER statement 16
multiple runs 56
reducing time 29, 210, 218, 254, 275, 280,
358, 368
results
plotting 145
printing 147
specifying 100
title 178
Simulation Runs 5
skew, parameters 85
SLOPE statement 411
SLOPETOL option 358
small-signal, DC sensitivity 159
source
AC sweep 9
DC sweep 32
SPARSE option 359
SPICE
compatibility 360
AC output 204
plot 330
SPICE option 360
SPMODEL option 361
START keyword 182
statement
PERIOD 401, 411
SLOPE 411
TDELAY 411
TFALL 411
TRISE 411
TSKIP 401
TUNIT, with TRISE statement 406, 407
statements
.AC 9
.ALIAS 14
HSPICE® Command Reference
X-2005.09
Index
T
.ALTER 16, 44
alter block 1
.BIASCHK 18
.CONNECT 23
.DATA 25
external file 25
inline 25
.DC 32, 35
.DCMATCH 38
.DCVOLT 40, 76
.DEL LIB 42
.DISTO 46
.DOUT 49
.EBD 52
.ELSE 54
.ELSEIF 55
.END 56
.ENDDATA 57
.ENDIF 58
.ENDL 59, 86
.ENDS 60, 61
.EOM 61
.FFT 62
.FOUR 65
.FSOPTIONS 66
.GLOBAL 68
.GRAPH 69
.HDL 71
.IBIS 72
.IC 40, 76
.ICM 78
.IF 79
.INCLUDE 54, 56, 79, 81, 157
.LAYERSTACK 82
.LIB 84, 86
nesting 86
.LOAD 91
.MACRO 93
.MALIAS 96
.MATERIAL 98
.MEASURE 100, 297, 301
.MODEL 123
.NET 129
.NODESET 131, 235
.NOISE 132
.OP 133
.OPTION SEARCH 356
.PARAM 137
HSPICE® Command Reference
X-2005.09
.PAT 141
.PKG 143
.PLOT 145
.PRINT 147
.PROBE 151
.PROTECT 153
.PZ 154
.SAMPLE 156
.SAVE 157
.SENS 159
.SHAPE 161
.STIM 167
.SUBCKT 172
.TEMP 175, 176
.TF 177
.TITLE 178
.TRAN 179
.UNPROTECT 184
.VEC 185
.WIDTH 186
STATFL option 362
statistics, listing 202
steatements
.ELSE 54
.STIM command 167
subcircuit commands 5
subcircuits
calling 93, 172
global versus local nodes 68
names 94, 174
node numbers 94, 174
parameter 60, 61, 93, 94, 172, 174
printing path numbers 324
test example 93, 172
.SUBCKT command 172
sweep
data 26, 301
frequency 10
inner 26
outer 26
SWEEP keyword 12, 36, 182
SYMB option 363
T
Tabular Data section
time interval 401
TARG_SPEC 101
435
Index
U
target specification 102
TDELAY statement 411
TEMP
keyword 12, 36
model parameter 176
.TEMP command 175
temperature
AC sweep 9
DC sweep 32, 33
derating 176
reference 176
.TF command 177
TFALL statement 411
threshold voltage 49
time 134
See also CPU time
TIMERES option 364
timestep
algorithms 254
calculation for DVDT=3 261
changing size 342
control 261, 345, 368
internal 249
maximum 274, 281, 349
minimum 275, 280, 350
reversal 200
setting initial 249
transient analysis algorithm 292
variation by HSPICE 249
.TITLE command 178
title for simulation 178
TNOM option 176, 365
TO keyword 113, 120
TOL keyword 156
TOP keyword 158
.TRAN command 179
transient analysis
Fourier analysis 65
initial conditions 40, 76
number of iterations 282
TRAP algorithm
See trapezoidal integration
trapezoidal integration
coefficient 307
TRCON option 366
TRIG keyword 101
TRIG_SPEC 101
trigger specification 102
436
TRISE statement 406, 407, 411
TRTOL option 368
TSKIP statement 401
TSTEP
multiplier 349, 350
option 349, 350
TUNIT statement 411
with TRISE statement 406, 407
U
U Element, transmission line model 124
UIC
keyword 182
parameter 40, 76
.UNPROTECT command 184
UNWRAP option 369
V
VAMODEL option 370
.VEC command 185
VERIFY option 371
Verilog-A commands 5
version
H9007 compatibility 271
HSPICE 128
Version Options 369, 370
VFLOOR option 372
Viewlogic graph data file 252
VIH statement 412
VIL statement 413
VNTOL option 259, 373
VOH statement 416, 418
voltage
error tolerance
DC analysis 344, 346
transient analysis 343
initial conditions 40, 76
iteration-to-iteration change 253
logic high 412, 416, 418
logic low 413
maximum change 200
minimum
DC analysis 201
listing 372
transient analysis 199
operating point table 134
HSPICE® Command Reference
X-2005.09
Index
W
relative change, setting 345
tolerance
MBYPASS multiplier 295
value for BYPASS 219
VOLTAGE keyword 134
VREF statement 420
VTH statement 421
W
W Elements transmission line model 124
WACC option 374
warnings
limiting repetitions 376
misuse of VERSION parameter 128
suppressing 316
WARNLIMIT option 376
WEIGHT keyword 113, 120
HSPICE® Command Reference
X-2005.09
WHEN keyword 108
WHEN, using with .MEASURE 107
.WIDTH command 186
WL option 377
WNFLAG option 375
WSF output data 221, 355
X
XDTEMP option 378
Y
YMAX parameter 120
YMIN parameter 119
Z
ZUKEN option 379
437
Index
Z
438
HSPICE® Command Reference
X-2005.09
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