HSPICE Simulation and Analysis User Guide

HSPICE Simulation and Analysis User Guide
HSPICE® Simulation and
Analysis User Guide
Version Y-2006.03, March 2006
Copyright Notice and Proprietary Information
Copyright © 2006 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, 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 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® Simulation and Analysis User Guide, Y-2006.03
ii
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Contents
1.
2.
Inside This Manual. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xxiii
The HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xxv
Other Related Publications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xxvi
Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xxvii
Customer Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xxviii
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1
HSPICE Varieties. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2
Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3
HSPICE Features for Running Higher-Level Simulations . . . . . . . . . . . . . . . .
5
Simulation Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5
Experimental Methods Supported by HSPICE . . . . . . . . . . . . . . . . . . . .
5
HSPICE Data Flow. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7
Simulation Process Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9
Setup and Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11
Setting Environment Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11
Setting License Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
License Queuing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11
12
Standard Input Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13
Design and File Naming Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . .
13
Output Configuration File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14
Initialization File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14
DC Operating Point Initial Conditions File . . . . . . . . . . . . . . . . . . . . . . . .
14
Input Netlist File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
Library Input File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
Analog Transition Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
Standard Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15
AC Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
AC Analysis Measurement Reults File . . . . . . . . . . . . . . . . . . . . . . . . . . .
16
iii
Contents
3.
iv
DC Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
DC Analysis Measurement Results File. . . . . . . . . . . . . . . . . . . . . . . . . .
17
Digital Output File. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
FFT Analysis Graph Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
Hardcopy Graph Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
Operating Point Information File. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17
Operating Point Node Voltages File . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
Output Listing File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18
Output Status File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
Output Tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
Subcircuit Cross-Listing File. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
Transient Analysis Measurement Results File . . . . . . . . . . . . . . . . . . . . .
19
Transient Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19
Running HSPICE Simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
20
Running HSPICE RF Simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
22
Running HSPICE Interactively . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
23
To Start Interactive Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
23
To Run a Command File in Interactive Mode . . . . . . . . . . . . . . . . . . . . . .
24
To Quit Interactive Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
24
Running Multithreading HSPICE Simulations . . . . . . . . . . . . . . . . . . . . . . . . .
24
To Run Multithreading . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Performance Improvement Estimations . . . . . . . . . . . . . . . . . . . . . .
24
25
Using HSPICE in Client/Server Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
26
To Start Client/Server Mode. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Server. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Client . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
26
26
27
To Simulate a Netlist in Client/Server Mode. . . . . . . . . . . . . . . . . . . . . . .
27
To Quit Client/Server Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
28
Running HSPICE to Calculate New Measurements . . . . . . . . . . . . . . . . . . . .
28
To Calculate New Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
28
Input Netlist and Data Entry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
29
Input Netlist File Guidelines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
29
Input Line Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
First Character . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
30
31
Delimiters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
32
Node Identifiers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
32
Contents
Instance Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
32
Hierarchy Paths . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
34
Numbers. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
34
Parameters and Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
36
Input Netlist File Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
36
Schematic Netlists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
37
Input Netlist File Composition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
39
Title of Simulation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
40
Comments and Line Continuation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
40
Element and Source Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
41
Defining Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
44
Node Naming Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Wildcards on Node Names . . . . . . . . . . . . . . . . . . . . . . . . . .
44
45
Element, Instance, and Subcircuit Naming Conventions . . . . . . . . . . . . .
47
Subcircuit Node Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
47
Path Names of Subcircuit Nodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
48
Abbreviated Subcircuit Node Names . . . . . . . . . . . . . . . . . . . . . . . . . . . .
48
Automatic Node Name Generation . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
49
Global Node Names. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
49
Circuit Temperature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
50
Data-Driven Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
50
Library Calls and Definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Library Building Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
51
51
Automatic Library Selection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
51
Defining Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Predefined Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Measurement Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
52
52
53
Altering Design Variables and Subcircuits . . . . . . . . . . . . . . . . . . . . . . .
Using Multiple .ALTER Blocks . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
53
54
Connecting Nodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
54
Deleting a Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
55
Ending a Netlist . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
55
Condition-Controlled Netlists (IF-ELSE). . . . . . . . . . . . . . . . . . . . . . . . . .
55
Using Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
57
Hierarchical Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
M (Multiply) Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
S (Scale) Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Hierarchical Parameters to Simplify Simulation . . . . . . . . . . .
58
58
59
59
Undefined Subcircuit Search . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
60
v
Contents
4.
vi
Subcircuit Call Statement Discrete Device Libraries. . . . . . . . . . . . . . . . . . . .
60
DDL Library Access . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
61
Vendor Libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
62
Subcircuit Library Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
63
Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
65
Passive Elements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
65
Values for Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
65
Resistor Elements in a HSPICE or HSPICE RF Netlist . . . . . . . . . . . . . .
Linear Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Behavioral Resistors in HSPICE or HSPICE RF . . . . . . . . . . . . . . .
Frequency-Dependent Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . .
Skin Effect Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
66
68
69
70
71
Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Linear Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency-Dependent Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . .
Behavioral Capacitors in HSPICE or HSPICE RF . . . . . . . . . . . . . .
DC Block Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Charge-Conserved Capacitors. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
71
74
75
76
76
77
Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Mutual Inductors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ideal Transformer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Linear Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency-Dependent Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . .
AC Choke Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Reluctors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
78
81
83
85
86
87
88
Active Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
91
Diode Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
91
Bipolar Junction Transistor (BJT) Element . . . . . . . . . . . . . . . . . . . . . . . .
93
JFETs and MESFETs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
95
MOSFETs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
97
Transmission Lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
100
W Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
W Element Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
100
101
Lossless (T Element) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ideal Transmission Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
105
107
Lossy (U Element) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
109
Frequency-Dependent Multi-Terminal S Element . . . . . . . . . . . . . . . . . .
110
Frequency Table Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
116
Group Delay Handler in Time Domain Analysis . . . . . . . . . . . . . . . . . . . .
116
Contents
5.
Preconditioning S Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
117
IBIS Buffers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
118
Sources and Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
119
Independent Source Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
119
Source Element Conventions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
119
Independent Source Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
120
DC Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
123
AC Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
123
Transient Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
124
Mixed Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
124
Port Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
125
Independent Source Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
129
Trapezoidal Pulse Source . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
129
Sinusoidal Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
133
Exponential Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
136
Piecewise Linear Source . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
General Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
MSINC and ASPEC Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Data-Driven Piecewise Linear Source . . . . . . . . . . . . . . . . . . . . . . .
139
139
139
142
Single-Frequency FM Source . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
143
Single-Frequency AM Source . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pattern Source . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
145
148
Pseudo Random-Bit Generator Source . . . . . . . . . . . . . . . . . . . . . . . . . .
153
Linear Feedback Shift Register . . . . . . . . . . . . . . . . . . . . . . . . . . . .
155
Conventions for F . 0 . . . . .8( . .)-5.8( 001 So)vTr poupo ificor1862(i)19.2(v) So4-6( . -5.8( . .
vii
Contents
viii
Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Multi-Input Gates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Laplace Transform . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pole-Zero Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency Response Table . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Foster Pole-Residue Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Behavioral Voltage Source (Noise Model) . . . . . . . . . . . . . . . . . . . .
Ideal Op-Amp . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ideal Transformer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
E Element Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
166
166
166
166
166
167
168
169
170
171
172
172
173
E Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ideal OpAmp . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Voltage Summer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Polynomial Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Zero-Delay Inverter Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Ideal Transformer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Voltage-Controlled Oscillator (VCO). . . . . . . . . . . . . . . . . . . . . . . . .
176
176
176
177
177
177
177
Using the E Element for AC Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . .
179
Current-Dependent Current Sources — F Elements . . . . . . . . . . . . . . . . . . . .
180
Current-Controlled Current Source (CCCS) Syntax. . . . . . . . . . . . . . . . .
Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Multi-Input Gates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
F Element Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
F Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
180
180
180
180
180
181
181
183
Voltage-Dependent Current Sources — G Elements. . . . . . . . . . . . . . . . . . . .
184
Voltage-Controlled Current Source (VCCS) . . . . . . . . . . . . . . . . . . . . . . .
Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Multi-Input Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Laplace Transform . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Pole-Zero Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Frequency Response Table . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Foster Pole-Residue Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
184
184
184
185
185
185
185
185
185
186
Behavioral Current Source (Noise Model) . . . . . . . . . . . . . . . . . . . . . . . .
186
Voltage-Controlled Resistor (VCR) . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
187
Contents
Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Multi-Input Gates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
187
187
188
188
Voltage-Controlled Capacitor (VCCAP) . . . . . . . . . . . . . . . . . . . . . . . . . .
NPWL Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PPWL Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
G Element Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
188
189
189
189
G Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Switch. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Switch-Level MOSFET . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Voltage-Controlled Capacitor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Zero-Delay Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Diode Equation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Diode Breakdown . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Triodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Behavioral Noise Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
192
192
192
193
193
193
193
194
194
194
Current-Dependent Voltage Sources — H Elements. . . . . . . . . . . . . . . . . . . .
195
Current-Controlled Voltage Source (CCVS) . . . . . . . . . . . . . . . . . . . . . . .
Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Multi-Input Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
195
195
195
195
195
195
Digital and Mixed Mode Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
199
U Element Digital Input Elements and Models. . . . . . . . . . . . . . . . . . . . .
General Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Model Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Digital-to-Analog Input Model Parameters . . . . . . . . . . . . . . . . . . . .
199
200
200
200
U Element Digital Outputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Model Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Analog-to-Digital Output Model Parameters. . . . . . . . . . . . . . . . . . .
203
203
203
Replacing Sources With Digital Inputs. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
206
Specifying a Digital Vector File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
210
Commands in a Digital Vector File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
211
Vector Patterns. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
211
Defining Tabular Data. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Input Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Expected Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Verilog Value Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Periodic Tabular Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
211
212
213
214
215
ix
Contents
6.
7.
x
Waveform Characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
216
Modifying Waveform Characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . .
216
Using the Context-Based Control Option . . . . . . . . . . . . . . . . . . . . . . . . .
217
Comment Lines and Line Continuations . . . . . . . . . . . . . . . . . . . . . . . . .
218
Parameter Usage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
First Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Second Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Third Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
218
218
219
219
Digital Vector File Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
220
Parameters and Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
223
Using Parameters in Simulation (.PARAM) . . . . . . . . . . . . . . . . . . . . . . . . . . .
223
Defining Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
223
Assigning Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Inline Parameter Assignments . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Parameters in Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
225
226
226
User-Defined Function Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
226
Predefined Analysis Function. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
227
Measurement Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
227
.PRINT, .PROBE, .PLOT, and .GRAPH Parameters . . . . . . . . . . . . . . . .
227
Multiply Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
227
Using Algebraic Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
228
Built-In Functions and Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
229
Parameter Scoping and Passing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
233
Library Integrity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
234
Reusing Cells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
234
Creating Parameters in a Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
234
String Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
237
Parameter Defaults and Inheritance. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Parameter Passing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
238
239
Parameter Passing Solutions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
240
Simulation Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
241
Overview of Output Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
241
Output Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
241
Output Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
242
Displaying Simulation Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
243
Contents
.PRINT Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Statement Order. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
243
244
.PLOT Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
244
.PROBE Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
245
.GRAPH Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
.MODEL Statement for .GRAPH . . . . . . . . . . . . . . . . . . . . . . . . . . .
245
246
Using Wildcards in PRINT, PROBE, PLOT, and GRAPH Statements . . .
Supported Wildcard Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . .
247
248
Print Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Changing the File Descriptor Limit . . . . . . . . . . . . . . . . . . . . . . . . . .
248
249
Printing the Subcircuit Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
249
Selecting Simulation Output Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
251
DC and Transient Output Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Nodal Capacitance Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Nodal Voltage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Current: Independent Voltage Sources . . . . . . . . . . . . . . . . . . . . . .
Current: Element Branches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Current: Subcircuit Pin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Power Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Print or Plot Power . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Diode Power Dissipation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
BJT Power Dissipation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
JFET Power Dissipation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
MOSFET Power Dissipation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
251
251
252
252
252
256
256
257
257
258
259
259
AC Analysis Output Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Nodal Capacitance Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Nodal Voltage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Current: Independent Voltage Sources . . . . . . . . . . . . . . . . . . . . . .
Current: Element Branches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Current: Subcircuit Pin . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Group Time Delay . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Network . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Noise and Distortion. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
260
261
261
263
263
264
264
265
266
Element Template Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
266
Specifying User-Defined Analysis (.MEASURE) . . . . . . . . . . . . . . . . . . . . . . .
267
.MEASURE Statement Order. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
268
.MEASURE Parameter Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
269
FIND and WHEN Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
270
Equation Evaluation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
270
Average, RMS, MIN, MAX, INTEG, and PP . . . . . . . . . . . . . . . . . . . . . . .
271
INTEGRAL Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
271
xi
Contents
8.
xii
DERIVATIVE Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
271
ERROR Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Error Equations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
272
272
Reusing Simulation Output as Input Stimuli. . . . . . . . . . . . . . . . . . . . . . . . . . .
274
Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
274
Element Template Listings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
275
Initializing DC/Operating Point Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . .
287
Simulation Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
287
Initialization and Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
288
DC Initialization and Operating Point Calculation . . . . . . . . . . . . . . . . . . . . . .
291
.OP Statement — Operating Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
291
291
Element Statement IC Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
292
Initial Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
293
SAVE and LOAD Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
.SAVE Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
.LOAD Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
294
294
295
.DC Statement—DC Sweeps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
295
Other DC Analysis Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
296
DC Initialization Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
296
Accuracy and Convergence . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
297
Accuracy Tolerances . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
297
Accuracy Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
299
Autoconverge Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
DCON and GMINDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
300
302
Reducing DC Errors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
304
Shorted Element Nodes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
306
Inserting Conductance, Using DCSTEP . . . . . . . . . . . . . . . . . . . . . . . . .
306
Floating-Point Overflow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
307
Diagnosing Convergence Problems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
307
Non-Convergence Diagnostic Table . . . . . . . . . . . . . . . . . . . . . . . . . . . .
308
Traceback of Non-Convergence Source . . . . . . . . . . . . . . . . . . . . . . . . .
309
Solutions for Non-Convergent Circuits . . . . . . . . . . . . . . . . . . . . . . . . . .
Poor Initial Conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Inappropriate Model Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . .
310
310
311
Contents
9.
PN Junctions (Diodes, MOSFETs, BJTs). . . . . . . . . . . . . . . . . . . . .
313
Transient Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
315
Simulation Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
315
Overview of Transient Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
316
Transient Analysis Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
317
Transient Analysis of an RC Network. . . . . . . . . . . . . . . . . . . . . . . . . . . .
318
Transient Analysis of an Inverter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
320
Using the .BIASCHK Statement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
321
Data Checking Methods. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Limit and Noise Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Maximum Method. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Minimum Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Region Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
322
322
323
323
324
Transient Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
325
Matrix Manipulation Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
326
Simulation Speed and Accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
327
Simulation Speed . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
327
Simulation Accuracy. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Timestep Control for Accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Models and Accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Guidelines for Choosing Accuracy Options . . . . . . . . . . . . . . . . . . .
327
328
329
329
Numerical Integration Algorithm Controls . . . . . . . . . . . . . . . . . . . . . . . . . . . .
330
Gear and Trapezoidal Algorithms. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
330
Numerical Integration Algorithm Controls (HSPICE RF) . . . . . . . . . . . . . . . . .
333
Selecting Timestep Control Algorithms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
333
Iteration Count Dynamic Timestep. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
334
Local Truncation Error Dynamic Timestep . . . . . . . . . . . . . . . . . . . . . . . .
334
DVDT Dynamic Timestep. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
335
Timestep Controls in HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Effect of TSTEP on Timestep Size Selection . . . . . . . . . . . . . . . . . .
336
337
Timestep Controls in HSPICE RF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
338
Fourier Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
338
Accuracy and DELMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
340
Fourier Equation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
340
xiii
Contents
xiv
10. AC Sweep and Small Signal Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
343
Using the .AC Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
343
.AC Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
343
AC Small Signal Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
344
AC Analysis of an RC Network . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
346
Other AC Analysis Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
348
Using .DISTO for Small-Signal Distortion Analysis . . . . . . . . . . . . . . . . .
349
Using .NOISE for Small-Signal Noise Analysis . . . . . . . . . . . . . . . . . . . .
349
Using .SAMPLE for Noise Folding Analysis . . . . . . . . . . . . . . . . . . . . . . .
350
11. Linear Network Parameter Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
351
.LIN Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
351
Identifying Ports with the Port Element . . . . . . . . . . . . . . . . . . . . . . . . . .
352
Using the P (Port) Element for Mixed-Mode Measurement . . . . . . . . . . .
356
.LIN Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
356
.LIN Output Syntax. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
.PRINT and .PROBE Statements. . . . . . . . . . . . . . . . . . . . . . . . . . .
Hybrid Parameter Calculations. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
357
357
359
Multi-Port Scattering (S) Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . .
360
Two-Port Transfer and Noise Calculations . . . . . . . . . . . . . . . . . . . . . . . .
Equivalent Input Noise Voltage and Current. . . . . . . . . . . . . . . . . . .
Equivalent Noise Resistance and Conductance . . . . . . . . . . . . . . .
Noise Correlation Impedance and Admittance. . . . . . . . . . . . . . . . .
Optimum Matching for Noise . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Noise Figure and Minimum Noise Figure . . . . . . . . . . . . . . . . . . . . .
Associated Gain . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Output Format for Group Delay in .sc* Files. . . . . . . . . . . . . . . . . . .
Output Format for Two-Port Noise Parameters in .sc* Files . . . . . . .
361
361
362
362
362
362
363
363
363
Noise Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
364
Hybrid (H) Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
365
Group Delay . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
366
RF Measurements From .LIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
367
Impedance Characterizations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
367
Stability Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
367
Gain Measurements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
367
Matching for Optimal Gain . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
368
Noise Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
368
Contents
Two-Port Transfer and Noise Measurements . . . . . . . . . . . . . . . . . . . . . .
369
Output Format for Two-Port Noise Parameters in .sc* Files. . . . . . . . . . .
VSWR. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
ZIN(i) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
YIN(i) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
K_STABILITY_FACTOR (Rollett Stability Factor) . . . . . . . . . . . . . . .
MU_STABILITY_FACTOR (Edwards-Sinsky Stability Factor) . . . . .
Maximum Available Power Gain—G_MAX. . . . . . . . . . . . . . . . . . . .
Maximum Stable Gain - G_MSG . . . . . . . . . . . . . . . . . . . . . . . . . . .
Maximum Unilateral Transducer Power Gain —G_TUMAX . . . . . . .
Unilateral Power Gain—GU . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Simultaneous Conjugate Match for G_MAX. . . . . . . . . . . . . . . . . . .
Equivalent Input Noise Voltage and Current—IN2, VN2, RHON . . .
Equivalent Noise Resistance and Conductance—RN, GN . . . . . . .
Noise Correlation Impedance and Admittance—ZCOR, YCOR. . . .
ZOPT, YOPT, GAMMA_OPT – Optimum Matching for Noise. . . . . .
Noise Figure and Noise Figure Minimum—NF, NFMIN . . . . . . . . . .
Associated Gain—G_As. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
369
370
370
370
370
371
371
371
372
372
373
374
374
375
375
375
376
Extracting Mixed-Mode Scattering (S) Parameters . . . . . . . . . . . . . . . . . . . . .
377
Defaults . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
378
Output File Formats . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
379
Two-Port Parameter Measurement . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
379
Output Format and Description . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
379
Features Supported . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
380
Prerequisites and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
381
Reported Statistics for the Performance Log (HSPICE RF Only) . . . . . .
381
Errors and Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
381
.NET Parameter Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
382
Network Analysis Example: Bipolar Transistor. . . . . . . . . . . . . . . . . . . . .
385
.NET Parameter Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
387
Bandpass Netlist: Network Analysis Results . . . . . . . . . . . . . . . . . . . . . .
388
References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
391
12. Using Verilog-A . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
393
Getting Started. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
394
Introduction to Verilog-A. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
397
xv
Contents
Mathematical Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
xvi
401
Transcendental Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
402
AC Analysis Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
403
Noise Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
403
Analog Events . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
403
Timestep and Simulator Control. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
404
System Tasks and I/O Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
404
Simulator Environment Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
405
Module Hierarchy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
406
Parameter Sets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
406
Simulation with Verilog-A Modules. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
407
Loading Verilog-A Devices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
407
Verilog-A File Search Path . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
408
Verilog-A File Loading Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . .
409
Instantiating Verilog-A Devices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
409
Using Model Cards with Verilog-A Modules . . . . . . . . . . . . . . . . . . . . . . .
410
Restrictions on Verilog-A Module Names. . . . . . . . . . . . . . . . . . . . . . . . .
412
Overriding Subcircuits with Verilog-A Modules . . . . . . . . . . . . . . . . . . . .
Netlist Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Command-line Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
412
412
413
Disabling .OPTION vamodel with .OPTION spmodel . . . . . . . . . . . . . . .
413
Using Vector Buses or "Ports" . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
414
Using Integer Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
415
Implicit Parameter M Support. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
415
Module and Parameter Name Case Sensitivity . . . . . . . . . . . . . . . . . . . .
Module Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Module Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
415
415
416
Output Simulation Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
416
V() and I() Access Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
417
Output Bus Signals . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
418
Output Internal Module Variables (HSPICE only) . . . . . . . . . . . . . . . . . .
419
Output Module Parameters (HSPICE only) . . . . . . . . . . . . . . . . . . . . . . .
419
Case Sensitivity in Simulation Data Output . . . . . . . . . . . . . . . . . . . . . . .
419
Using Wildcards in Verilog-A (HSPICE only) . . . . . . . . . . . . . . . . . . . . . .
420
Port Probing and Branch Current Reporting Conventions . . . . . . . . . . . .
421
Unsupported Output Function Features. . . . . . . . . . . . . . . . . . . . . . . . . .
421
Using the Stand-alone Compiler . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
421
Setting Environment Option for HSPICE Verilog-A Compiler. . . . . . . . . . . . . .
422
Contents
The Compiled Model Library Cache . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
422
Cache Location . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
423
Deleting the Cache. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
423
Unsupported Language Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
424
Known Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
428
analysis() Function Behavior . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
428
13. Simulating Variability. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
431
Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
431
How To Define Variability in HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
431
Variation Blocks Replace Previous Approaches . . . . . . . . . . . . . . . . . . . . . . .
432
14. Variation Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
433
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
433
Variation Block Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
434
General Section . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
434
435
Global and Local Variations Sub-Blocks . . . . . . . . . . . . . . . . . . . . . . . . .
Independent Random Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Dependent Random Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Variations of Model Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Variations of Element Parameters . . . . . . . . . . . . . . . . . . . . . . . . . .
Absolute Versus Relative Variation. . . . . . . . . . . . . . . . . . . . . . . . . .
Access Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
435
436
437
438
439
442
442
Variation Block Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
443
15. Monte Carlo Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
445
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
445
Monte Carlo Analysis in HSPICE. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
447
Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
448
Variation Block Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
450
Simulation Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
451
Application Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
453
xvii
Contents
xviii
16. DC Mismatch Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
455
Mismatch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
455
DCmatch Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
455
Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
456
DCmatch Table Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
458
Output From .PROBE and .MEASURE Commands . . . . . . . . . . . . . . . .
Syntax for .PROBE Command . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Syntax for .MEASURE Command . . . . . . . . . . . . . . . . . . . . . . . . . .
460
460
461
Practical Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
DCmatch Variability as a Function of Device Geometry. . . . . . . . . .
Parameter Traceability . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
461
461
462
Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
463
References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
464
17. Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
465
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
465
Optimization Control. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
466
Simulation Accuracy. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
466
Curve Fit Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
467
Goal Optimization. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
467
Timing Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
467
Optimization Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Optimizing Analysis (.DC, .TRAN, .AC) . . . . . . . . . . . . . . . . . . . . . .
468
469
Optimization Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
MOS Level 3 Model DC Optimization. . . . . . . . . . . . . . . . . . . . . . . .
MOS Level 13 Model DC Optimization. . . . . . . . . . . . . . . . . . . . . . .
RC Network Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Optimizing CMOS Tristate Buffer . . . . . . . . . . . . . . . . . . . . . . . . . . .
BJT S Parameters Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . .
BJT Model DC Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Optimizing GaAsFET Model DC. . . . . . . . . . . . . . . . . . . . . . . . . . . .
Optimizing MOS Op-amp . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
470
470
473
476
481
485
487
489
493
18. RC Reduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
499
Linear Acceleration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
499
PACT Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
500
PI Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
501
Contents
Linear Acceleration Control Options Summary . . . . . . . . . . . . . . . . . . . . . . . .
501
19. Running Demonstration Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
505
Using the Demo Directory Tree . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
505
Two-Bit Adder Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
506
One-Bit Subcircuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
506
MOS Two-Bit Adder Input File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
508
MOS I-V and C-V Plotting Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
508
Plotting Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
509
MOS I-V and C-V Plot Example Input File . . . . . . . . . . . . . . . . . . . . . . . .
513
CMOS Output Driver Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
513
Strategy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
514
CMOS Output Driver Example Input File . . . . . . . . . . . . . . . . . . . . . . . . .
518
Temperature Coefficients Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
518
Input File for Optimized Temperature Coefficients . . . . . . . . . . . . . . . . . .
519
Optimization Section . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
520
Simulating Electrical Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
520
T2N2222 Optimization Example Input File. . . . . . . . . . . . . . . . . . . . . . . .
521
Modeling Wide-Channel MOS Transistors . . . . . . . . . . . . . . . . . . . . . . . . . . . .
521
Demonstration Input Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
524
Statistical Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
543
Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
543
Application of Statistical Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
544
Analytical Model Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
544
Simulating Circuit and Model Temperatures . . . . . . . . . . . . . . . . . . . . . . . . . .
545
Temperature Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
547
.TEMP Statement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
548
Worst Case Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
548
Model Skew Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Skew Parameters in HSPICE . . . . . . . . . . . . . . . . . . . . . . . . .
Skew File Interface to Device Models. . . . . . . . . . . . . . . . . . . . . . . .
548
550
552
Monte Carlo Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
553
Monte Carlo Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
554
A.
xix
Contents
B.
xx
Monte Carlo Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
556
.PARAM Distribution Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
556
Monte Carlo Parameter Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
559
Monte Carlo Examples. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Gaussian, Uniform, and Limit Functions . . . . . . . . . . . . . . . . . . . . .
Major and Minor Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
RC Time Constant . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Switched Capacitor Filter Design . . . . . . . . . . . . . . . . . . . . . . . . . . .
560
560
563
565
566
Worst Case and Monte Carlo Sweep Example . . . . . . . . . . . . . . . . . . . . . . . .
568
Transient Sigma Sweep Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
570
Monte Carlo Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
571
Simulating the Effects of Global and Local Variations with Monte Carlo . . . . .
578
Variations Specified on Geometrical Instance Parameters . . . . . . . . . . .
578
Variations Specified in the Context of Subcircuits . . . . . . . . . . . . . . . . . .
580
Variations on a Model Parameter Using a Local Model in Subcircuit. . . .
581
Indirect Variations on a Model Parameter . . . . . . . . . . . . . . . . . . . . . . . .
581
Variations Specified on Model Parameters . . . . . . . . . . . . . . . . . . . . . . .
582
Variations Specified Using DEV and LOT . . . . . . . . . . . . . . . . . . . . . . . .
583
Combinations of Variation Specifications . . . . . . . . . . . . . . . . . . . . . . . . .
583
Variation on Model Parameters as a Function of Device Geometry. . . . .
584
Conclusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
585
Full Simulation Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
587
Simulation Example Using AvanWaves . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
587
Input Netlist and Circuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
587
Execution and Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example.ic . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example.lis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Example.st0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
589
590
590
593
Simulation Graphical Output in AvanWaves. . . . . . . . . . . . . . . . . . . . . . .
596
Simulation Example Using CosmosScope. . . . . . . . . . . . . . . . . . . . . . . . . . . .
602
Input Netlist and Circuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
602
Execution and Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
604
View HSPICE Results in CosmosScope . . . . . . . . . . . . . . . . . . . . . . . . .
Viewing HSPICE Transient Analysis Waveforms . . . . . . . . . . . . . . .
Viewing HSPICE AC Analysis Waveforms . . . . . . . . . . . . . . . . . . . .
Viewing HSPICE DC Analysis Waveforms . . . . . . . . . . . . . . . . . . . .
605
605
607
609
Contents
C.
HSPICE GUI for Windows . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
611
Working with Designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
611
Configuring the HSPICE GUI for Windows . . . . . . . . . . . . . . . . . . . . . . . . . . .
613
Running Multiple Simulations. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
614
Building the Batch Job List. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
615
Simulating the Batch Job List. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
616
Using the Drag-and-drop Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
616
Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
617
xxi
Contents
xxii
About This Manual
This manual describes how to use HSPICE 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, Overview
Describes HSPICE features and the simulation
process.
Chapter 2, Setup and
Simulation
Describes the environment variables, standard I/O
files, invocation commands, and simulation
modes.
Chapter 3, Input Netlist and
Data Entry
Describes the input netlist file and methods of
entering data.
Chapter 4, Elements
Describes the syntax for the basic elements of a
circuit netlist in HSPICE or HSPICE RF.
Chapter 5, Sources and
Stimuli
Describes element and model statements for
independent sources, dependent sources,
analog-to-digital elements, and digital-to-analog
elements.
Chapter 6, Parameters and
Functions
Describes how to use parameters within an
HSPICE netlist.
Chapter 7, Simulation
Output
Describes how to use output format statements
and variables to display steady state, frequency,
and time domain simulation results.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
xxiii
About This Manual
Inside This Manual
xxiv
Chapter
Description
Chapter 8, Initializing DC/
Operating Point Analysis
Describes DC initialization and operating point
analysis.
Chapter 9, Transient
Analysis
Describes how to use transient analysis to
compute the circuit solution.
Chapter 10, AC Sweep and
Small Signal Analysis
Describes how to perform AC sweep and small
signal analysis.
Chapter 11, Linear Network
Parameter Analysis
Describes how to perform an AC sweep to extract
small-signal linear network parameters.
Chapter 12, Using VerilogA
Describes how to use Verilog-A in HSPICE
simulations.
Chapter 13, Simulating
Variability
Introduces variability, describes how it is defined in
HSPICE, and introduces the variation block.
Chapter 14, Variation Block
Describes the use model and structure of the
variation block.
Chapter 15, Monte Carlo
Analysis
Describes Monte Carlo analysis in HSPICE.
Chapter 16, DC Mismatch
Analysis
Describes the use of DCmatch analysis.
Chapter 17, Optimization
Describes optimization in HSPICE for optimizing
electrical yield.
Chapter 18, RC Reduction
Describes RC network reduction.
Chapter 19, Running
Demonstration Files
Contains examples of basic file construction
techniques, advanced features, and simulation
tricks. Lists and describes several HSPICE and
HSPICE RF input files.
Appendix A, Statistical
Analysis
Describes the features available in HSPICE for
statistical analysis before the Y-2006.03 release.
Appendix B, Full Simulation
Examples
Contains information and sample input netlists for
two full simulation examples.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
About This Manual
The HSPICE Documentation Set
Chapter
Description
Appendix C, HSPICE GUI
for Windows
Describes how to use the HSPICE GUI for
Windows.
The HSPICE Documentation Set
This manual is a part of the HSPICE documentation set, which includes the
following manuals:
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 highspeed circuit design.
AvanWaves User Guide
Describes the AvanWaves tool, which you can use to
display waveforms generated during HSPICE circuit
design simulation.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
xxv
About This Manual
Other Related Publications
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/ReleaseNotes) 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:
xxvi
■
The HSPICE Release Notes, available on SolvNet (see Known Limitations
and Resolved STARs, below)
■
Documentation on the Web, which provides PDF documents and is
available through SolvNet at http://solvnet.synopsys.com/DocsOnWeb
■
The Synopsys MediaDocs Shop, from which you can order printed copies
of Synopsys documents, at http://mediadocs.synopsys.com
HSPICE® Simulation and Analysis User Guide
Y-2006.03
About This Manual
Conventions
You might also want to refer to the documentation for the following related
Synopsys products:
■
CosmosScope
■
Aurora
■
Raphael
■
VCS
Known Limitations and Resolved STARs
You can find information about known problems and limitations and resolved
Synopsys Technical Action Requests (STARs) in the HSPICE Release Notes in
SolvNet.
To see the HSPICE Release Notes:
1. Go to https://solvnet.synopsys.com/ReleaseNotes. (If prompted, enter your
user name and password. If you do not have a Synopsys user name and
password, follow the instructions to register with SolvNet.)
2. Click HSPICE, then click the release you want in the list that appears at the
bottom.
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]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
xxvii
About This Manual
Customer Support
Convention
Description
...
Indicates that parameters can be repeated as many times as
necessary:
pin1 pin2 ... pinN
|
Indicates a choice among alternatives, such as
low | medium | high
\
Indicates a continuation of a command line.
/
Indicates levels of directory structure.
Edit > Copy
Indicates a path to a menu command, such as opening the
Edit menu and choosing Copy.
Control-c
Indicates a keyboard combination, such as holding down the
Control key and pressing c.
Customer Support
Customer support is available through SolvNet online customer support and
through contacting the Synopsys Technical Support Center.
Accessing SolvNet
SolvNet includes an electronic knowledge base of technical articles and
answers to frequently asked questions about Synopsys tools. SolvNet also
gives you access to a wide range of Synopsys online services, which include
downloading software, viewing Documentation on the Web, and entering a call
to the Support Center.
To access SolvNet:
1. Go to the SolvNet Web page at http://solvnet.synopsys.com.
2. If prompted, enter your user name and password. (If you do not have a
Synopsys user name and password, follow the instructions to register with
SolvNet.)
If you need help using SolvNet, click Help on the SolvNet menu bar.
xxviii
HSPICE® Simulation and Analysis User Guide
Y-2006.03
About This Manual
Customer Support
Contacting the Synopsys Technical Support Center
If you have problems, questions, or suggestions, you can contact the Synopsys
Technical Support Center in the following ways:
■
Open a call to your local support center from the Web by going to
http://solvnet.synopsys.com/EnterACall (Synopsys user name and
password required).
■
Send an e-mail message to your local support center.
■
•
E-mail [email protected] from within North America.
•
Find other local support center e-mail addresses at
http://www.synopsys.com/support/support_ctr.
Telephone your local support center.
•
Call (800) 245-8005 from within the continental United States.
•
Call (650) 584-4200 from Canada.
•
Find other local support center telephone numbers at
http://www.synopsys.com/support/support_ctr.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
xxix
About This Manual
Customer Support
xxx
HSPICE® Simulation and Analysis User Guide
Y-2006.03
1
Overview
1
Describes HSPICE features and the simulation process.
Synopsys HSPICE is an optimizing analog circuit simulator. You can use it to
simulate electrical circuits in steady-state, transient, and frequency domains.
HSPICE or HSPICE RF is unequalled for fast, accurate circuit and behavioral
simulation. It facilitates circuit-level analysis of performance and yield, by using
Monte Carlo, worst-case, parametric sweep, and data-table sweep analyses,
and employs the most reliable automatic-convergence capability (see
Figure 1).
Figure 1
Synopsys HSPICE or HSPICE RF Design Features
Transmission Line
Signal Integrity
Monte Carlo
Worst-Case Analysis
HSPICE
or
HSPICE RF
Circuit Cell
Optimization
Cell
Characterization
Photocurrent/
Radiation Effects
Incremental
Optimization
AC, DC,
Transient
HSPICE or HSPICE RF forms the cornerstone of a suite of Synopsys tools and
services that allows accurate calibration of logic and circuit model libraries to
actual silicon performance.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
1
Chapter 1: Overview
HSPICE Varieties
The size of the circuits that HSPICE or HSPICE RF can simulate is limited only
by memory. As a 32-bit application, HSPICE can address a maximum of 2Gb or
4Gb of memory, depending on your system.
For a description of commands that you can include in your HSPICE netlist,
see the “Netlist Commands” chapter in the HSPICE Command Reference.
HSPICE Varieties
Synopsys HSPICE is available in two varieties:
■
HSPICE
■
HSPICE RF
Like traditional SPICE simulators, HSPICE is Fortran-based, but it is faster and
has more capabilities than typical SPICE simulators. HSPICE accurately
simulates, analyzes, and optimizes circuits, from DC, to microwave frequencies
that are greater than 100 GHz. HSPICE is ideal for cell design and process
modeling. It is also the tool of choice for signal-integrity and transmission-line
analysis.
HSPICE RF is a newer, C++ version of the traditional Fortran-based HSPICE.
Many (but not all) HSPICE simulation capabilities have been implemented in
HSPICE RF, and HSPICE RF offers some new capabilities that are not in
available in traditional HSPICE.
HSPICE RF usually produces results at the desired level of accuracy in a
shorter time than HSPICE requires for the same level of accuracy. HSPICE RF
can also perform HSPICE simulations of radio-frequency (RF) devices, which
HSPICE does not support.
This guide describes all of the features that HSPICE supports. HSPICE RF
supports some—but not all—of these features as well. For descriptions of
HSPICE RF features and a list of the differences between HSPICE and
HSPICE RF, see the “HSPICE RF Features and Functionality” chapter in the
HSPICE RF User Guide.
2
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 1: Overview
Features
Features
Synopsys HSPICE or HSPICE RF is compatible with most SPICE variations,
and has the following additional features:
■
Superior convergence
■
Accurate modeling, including many foundry models
■
Hierarchical node naming and reference
■
Circuit optimization for models and cells, with incremental or simultaneous
multiparameter optimizations in AC, DC, and transient simulations
■
Interpreted Monte Carlo and worst-case design support
■
Input, output, and behavioral algebraics for cells with parameters
■
Cell characterization tools, to characterize standard cell libraries
■
Geometric lossy-coupled transmission lines for PCB, multi-chip, package,
and IC technologies
■
Discrete component, pin, package, and vendor IC libraries
■
Interactive graphing and analysis of multiple simulation waveforms by using
with AvanWaves and CosmosScope
■
Flexible license manager that allocates licenses intelligently based on run
status and user-specified job priorities you specify.
If you suspend a simulation job, the load sharing facility (LSF) license
manager signals HSPICE to release that job’s license. This frees the license
for another simulation job, or so the stopped job can reclaim the license and
resume. You can also prioritize simulation jobs you submit; LSF
automatically suspends low-priority simulation jobs to run high-priority jobs.
When the high-priority job completes, LSF releases the license back to the
lower-priority job, which resumes from where it was suspended.
■
A number of circuit analysis types (see Figure 2) and device modeling
technologies (see Figure 3).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
3
Chapter 1: Overview
Features
Figure 2
Synopsys HSPICE or HSPICE RF Circuit Analysis Types
Operating
Point
Parametric
Monte Carlo
Pole-Zero
HSPICE
or
HSPICE RF
Optimization
Monte Carlo
Data Driven
Frequency
Transient
S-parameter
Monte Carlo
Optimization
Optimization
Mixed
AC/Transient
Monte Carlo
Data Driven
Figure 3
Monte Carlo analysis
supported in
Synopsys HSPICE
only
Data Driven
Synopsys HSPICE Modeling Technologies
40+ Industrial and
Academic Models
SPICE
BJT
Magnetics
MOS
Common Model
Interface
Lossy
Transmission
Lines
Device Models
SOI
IBIS
Mixed Signal
JFET/GaAsFET
Diode
Tunnel Diode
4
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 1: Overview
HSPICE Features for Running Higher-Level Simulations
HSPICE Features for Running Higher-Level Simulations
Simulations at the integrated circuit level and at the system level require careful
planning of the organization and interaction between transistor models and
subcircuits. Methods that worked for small circuits might have too many
limitations when applied to higher-level simulations.
You can use the following HSPICE or HSPICE RF features to organize how
simulation circuits and models run:
■
Explicit include files – .INCLUDE statement.
■
Implicit include files – .OPTION SEARCH=‘lib_directory’ (HSPICE
only).
■
Algebraics and parameters for devices and models – .PARAM statement.
■
Parameter library files – .LIB statement.
■
Automatic model selector – LMIN, LMAX, WMIN, and WMAX model
parameters.
■
Parameter sweep – sweep analysis statements.
■
Statistical analysis – sweep monte analysis statements (HSPICE only).
■
Multiple alternative – .ALTER statement (HSPICE only).
■
Automatic measurements – .MEASURE statement.
■
Condition-controlled netlists (IF-ELSEIF-ELSE-ENDIF statements).
Simulation Structure
Experimental Methods Supported by HSPICE
Typically, you use experiments to analyze and verify complex designs. These
experiments can be simple sweeps, more complex Monte Carlo and
optimization analyses (HSPICE only), or setup and hold violation analyses of
DC, AC, and transient conditions.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
5
Chapter 1: Overview
Simulation Structure
Figure 4
Simulation Program Structure
Simulation Experiment
Single point
Analysis
Optimization
Initial
Conditions
Circuit
Transient
Sweep
Results
Analysis
Timing
Violations
Statistical
Worst Case
DC
Library
Stimuli
AC
Options
For each simulation experiment, you must specify tolerances and limits to
achieve the desired goals, such as optimizing or centering a design. Common
factors for each experiment are:
■
process
■
voltage
■
temperature
■
parasitics
HSPICE or HSPICE RF supports two experimental methods:
■
Single point – a simple procedure that produces a single result, or a single
set of output data.
■
Multipoint – performs an analysis (single point) sweep for each value in an
outer loop (multipoint) sweep.
The following are examples of multipoint experiments:
6
■
Process variation – Monte Carlo or worst-case model parameter variation
(HSPICE only).
■
Element variation – Monte Carlo (HSPICE only) or element parameter
sweeps.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 1: Overview
Simulation Structure
■
Voltage variation – VCC, VDD, or substrate supply variation.
■
Temperature variation – design temperature sensitivity.
■
Timing analysis – basic timing, jitter, and signal integrity analysis.
■
Parameter optimization – balancing complex constraints, such as speed
versus power, or frequency versus slew rate versus offset (analog circuits).
HSPICE Data Flow
HSPICE or HSPICE RF accepts input and simulation control information from
several different sources. They can output results in a number of convenient
forms for review and analysis. Figure 5 shows the overall data flow.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
7
Chapter 1: Overview
Simulation Structure
Figure 5
Overview of Data Flow
hspice.ini
Command line input
(initialization file)
meta.cfg
(output
configuration file)
<design>.sp
(netlist input file)
Models and
device libraries
command.inc
(command include
file – optional)
HSPICE
or
HSPICE RF
(simulation)
<design>.tr#
(graph data
output file)
AvanWaves
(graph and
analysis)
Other output files:
<design>.lis
<design>.mt#
<design>.sw#
<design>.ms#
<design>.ac#
<design>.ma#
<design>.gr#
<design>.pa#
<design>.st#
<design>.ft#
<design>.a2d
Graphics
hardcopy file
Printer or
plotter
8
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 1: Overview
Simulation Structure
To simulate a design in HSPICE, you do the following:
1. To begin design entry and simulation, create an input netlist file.
Most schematic editors and netlisters support the SPICE or HSPICE
hierarchical format.
2. HSPICE or HSPICE RF executes the analyses specified in the input file.
3. HSPICE or HSPICE RF stores the simulation results requested in either an
output listing file or (if you specified .OPTION POST) a graph data file.
If you specified POST, HSPICE or HSPICE RF stores the circuit solution (in
either steady state, time, or frequency domain).
4. To view or plot the results for any nodal voltage or branch current, use a
high-resolution graphic output terminal or laser printer.
HSPICE provides a complete set of print and plot variables for viewing
analysis results. HSPICE RF supports some, but not all, HSPICE print
variables.
The HSPICE or HSPICE RF programs include a textual command line
interface. For example, to execute the program, enter the hspice or
hspicext command, the input file name, and the desired options. You can use
the command line at the prompt in a Unix shell, or a Windows command
prompt, or (for HSPICE only) click on an icon in a Windows environment.
You can specify whether the HSPICE or HSPICE RF program simulation output
appears in an output listing file, or in a graph data file (HSPICE only). HSPICE
or HSPICE RF creates standard output files to describe initial conditions (.ic
extension) and output status (.st0 extension). In addition, HSPICE or HSPICE
RF creates various output files, in response to user-defined input options—for
example, HSPICE creates a <design>.tr0 file, in response to a .TRAN
transient analysis statement.
The default waveform display tool CosmosScope. See the CosmosScope User
Guide for instructions about how to use CosmosScope.
Simulation Process Overview
Figure 6 shows the HSPICE or HSPICE RF simulation process.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
9
Chapter 1: Overview
Simulation Structure
Figure 6
Simulation Process
1. Invocation
2. Run script
3. Licensing
Select version
Select best architecture
Run HSPICE
Find license file in
LM_LICENSE_FILE
Get FLEXlm license token
4. Simulation
configuration
Read ~/meta.cfg or
Read <installdir>/meta.cfg
5. Design input
Read input file: demo.sp
Open temp. files in $tmpdir
Open output file
Read hspice.ini file
6. Library input
Read .INCLUDE statement files
Read .LIB
Read implicit include (.inc) files
7. Operating point
initialization
Read .ic file (optional)
Find operating point
Write .ic file (optional)
8. Multipoint analysis
Open measure data files .mt0
Initialize outer loop sweep
Set analysis temperature
9. Single point analysis
Open graph data file .tr0
Perform analysis sweep
10. Worst case .ALTER
11. Clean up
10
hspice -i demo.sp -o demo.lis -OR- hspicerf -a ckt.in ckt
Process library delete/add
Process parameter and
topology changes
Close all files
Release all tokens
HSPICE® Simulation and Analysis User Guide
Y-2006.03
2
Setup and Simulation
2
Describes the environment variables, standard I/O files, invocation commands,
and simulation modes.
For descriptions of individual HSPICE commands mentioned in this chapter,
see the HSPICE Command Reference.
Setting Environment Variables
Before using HSPICE, you need to set these environment variables
■
LM_LICENSE_FILE—Specifies the path to the license file (required)
■
META_QUEUE—Enables HSPICE licenses to be queued
■
tmpdir (UNIX), TEMP or TMP (Windows)—Allows you to control the location
of the temporary files
Setting License Variables
HSPICE or HSPICE RF requires you to set the LM_LICENSE_FILE
environment variable. This variable specifies the full path to the license.dat
license file. Set the LM_LICENSE_FILE environment variable to point to the
HSPICE and HSPICE RF license file.
For example, if your HSPICE RF license file is in:
/usr/cad/hspicext/license.dat
And your HSPICE license file is in:
/usr/cad/hspice/license.dat
HSPICE® Simulation and Analysis User Guide
Y-2006.03
11
Chapter 2: Setup and Simulation
Setting Environment Variables
Then you would enter:
setenv LM_LICENSE_FILE /usr/cad/hspicext/license.dat:\
/usr/cad/hspice/license.dat
You can also set the variable [email protected] to point to a license file on a
server.
■
If you are using the C shell, add the following line to the .cshrc file:
setenv LM_LICENSE_FILE [email protected]
■
If you are using the Bash or Bourne shell, add these lines to the .bashrc or
.profile file:
[email protected]
export LM_LICENSE_FILE
The port and host name variables correspond to the TCP port and license
server host name specified in the SERVER line of the Synopsys license file.
Note:
To ensure better performance, it is recommended that you use
[email protected] rather than using the path to the license file.
Each license file can contain licenses for many packages from multiple
vendors. You can specify multiple license files by separating each entry. For
UNIX, use a colon (:) and for Windows, use a semicolon (;).
For details about setting license file environment variable, see “Setting Up
HSPICE for Each User” in the Installation Guide.
License Queuing
Setting the optional META_QUEUE environment variable to 1 enables HSPICE
licenses to be queued:
setenv META_QUEUE 1
The licensing queuing works as follows: If you have five HSPICE floating
licenses and all five licenses are checked out with the META_QUEUE
environment variable enabled, then the next job submitted waits in the queue
until a license is available (when one of the previous five jobs finishes). When
META_QUEUE is enabled and all available licenses are in use, an error message
is issued that says no licenses are available.
If you have more than one HSPICE token (INCREMENT line) and the version
dates are different, only the first token in your license file is queued. FLEXlm
12
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Standard Input Files
queues the first increment line that satisfies the request. If you have two
increment lines with different versions, two license pools are created on the
server. When you issue the queuing request, the server attempts to satisfy the
request, but if it is not possible, the server queues the first increment line that
satisfies the request. Once that particular increment line is queued, it waits for
that increment line to become free. The server does not continually look for any
other line that satisfies this request. This is normal operation for FLEXlm.
Standard Input Files
This section describes the standard input files to HSPICE or HSPICE RF.
Design and File Naming Conventions
The design name identifies the circuit and any related files, including:
■
Schematic and netlist files.
■
Simulator input and output files.
■
Design configuration files.
■
Hardcopy files.
HSPICE, HSPICE RF, and AvanWaves extract the design name from their input
files, and perform actions based on that name. For example, AvanWaves reads
the <design>.cfg configuration file to restore node setups used in previous
AvanWaves runs.
HSPICE, HSPICE RF, and AvanWaves read and write files related to the
current circuit design. Files related to a design usually reside in one directory.
The output file is stdout on Unix platforms, which you can redirect.
Table 1 lists input file types, and their standard names. The sections that follow
describe these files.
Table 1
Input Files
Input File Type
File Name
Output configuration file
meta.cfg
Initialization file
hspice.ini
DC operating point initial conditions file
<design>.ic#
HSPICE® Simulation and Analysis User Guide
Y-2006.03
13
Chapter 2: Setup and Simulation
Standard Input Files
Table 1
Input Files (Continued)
Input File Type
File Name
Input netlist file
<design>.sp
Library input file
<library_name>
Analog transition data file
<design>.d2a
Output Configuration File
You use the output configuration file to set up the printer, plotter, and terminal. It
includes a line (default_include=<filename>) to set up a path to the default .ini
file (for example, hspice.ini).
The default include filename is case-sensitive (except for the PC and Windows
versions of HSPICE).
Initialization File
You use the initialization file to specify user defaults. If the run directory
contains an hspice.ini file, HSPICE or HSPICE RF includes its contents at the
top of the input file.
To include initialization files, you can define default_include=<filename> in a
command.inc or meta.cfg file.
You can use an initialization file to set options (for .OPTION statements) and to
access libraries.
DC Operating Point Initial Conditions File
The DC operating point initial conditions file, <design>.ic#, is an optional input
file that contains initial DC conditions for particular nodes. You can use this file
to initialize DC conditions, by using either a .NODESET or an .IC statement.
A .SAVE statement can also create a <design>.ic# file. A subsequent .LOAD
statement initializes the circuit to the DC operating point values specified in this
file.
14
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Standard Output Files
Input Netlist File
The input netlist file, <design>.sp, contains the design netlist. Optionally, it can
also contain statements specifying the type of analysis to run, type of output
desired, and what library to use.
Library Input File
You use <library_name> files to identify libraries and macros that need to be
included for simulating <design>.sp.
Analog Transition Data File
When you run HSPICE in standalone mode, a <design>.d2a file contains state
information for a U Element mixed-mode simulation.
Standard Output Files
This section describes the standard output files from HSPICE. For informaton
about the standard output file from HSPICE RF, see section HSPICE RF
Output File Types in the HSPICE RF Manual. The various types of output files
produced are listed in Table 2.
Table 2
HSPICE Output Files and Suffixes
Output File Type
Extension
AC analysis measurement results
.ma#a
AC analysis results (from .POST statement)
.ac#
DC analysis measurement results
.ms#
DC analysis results (from .POST statement)
.sw#
Digital output
.a2d
FFT analysis graph data (from FFT statement)
.ft#
HSPICE® Simulation and Analysis User Guide
Y-2006.03
15
Chapter 2: Setup and Simulation
Standard Output Files
Table 2
HSPICE Output Files and Suffixes (Continued)
Output File Type
Extension
Hardcopy graph data (from meta.cfg
PRTDEFAULT)
.gr#b †
Operating point information (from .OPTION
OPFILE statement)
.dp#
Operating point node voltages (initial conditions) .ic#
Output listing
.lis, or user-specified
Output status
.st#
Output tables (from .DCMATCH OUTVAR
statement)
.dm#
Subcircuit cross-listing (HSPICE only; not
supported in HSPICE RF)
.pa#
Transient analysis measurement results
.mt#
Transient analysis results (from .POST
statement)
.tr#
a. # can be either a sweep number or a hardcopy file number. For .ac#, .dp#, .dm#,
.ic#, .st#, .sw#, and .tr# files, # is from 0 through 9999.
b. Requires a .GRAPH statement, or a pointer to a file in the meta.cfg file. The PC
version of HSPICE does not generate this file.
AC Analysis Results File
HSPICE writes AC analysis results to file <output_file>.ac#, where # is
0-9999, according to your specifications following the .AC statement. These
results list the output variables as a function of frequency.
AC Analysis Measurement Reults File
HSPICE writes AC analysis measurement results to file <output_file>.ma#
when the input file includes a .MEASURE AC statement.
16
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Standard Output Files
DC Analysis Results File
HSPICE writes DC analysis results to file <output_file>.sw#, where # is
0-9999, when the input file includes a .DC statement. This file contains the
results of the applied stepped or swept DC parameters defined in that
statement. The results can include noise, distortion, or network analysis.
DC Analysis Measurement Results File
HSPICE writes DC analysis measurement results to file <output_file>.ms#
when the input file includes a .MEASURE DC statement.
Digital Output File
The digital output file, <design>.a2d, contains data that the A2D conversion
option of the U element converted to digital form.
FFT Analysis Graph Data File
The FFT analysis graph data file, <output_file>.ft#, contains the
graphical data needed to display the FFT analysis waveforms.
Hardcopy Graph Data File
HSPICE writes hardcopy graph data to file <output_file>.gr# when the
input file includes a .GRAPH statement. The file produced is in the form of a
printer file, typically in Adobe PostScript or HP PCL format. This facility is not
available in the PC version of HSPICE.
Operating Point Information File
HSPICE writes operating point information to file <design>.dp# when the input
file includes an .OPTION OPFILE=1 statement.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
17
Chapter 2: Setup and Simulation
Standard Output Files
Operating Point Node Voltages File
HSPICE writes operati.96 T67350 0 TD0.0024 Tc-0.0151 Tw[ingpo(intnNodev)2li.96 27.650 0
18
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Standard Output Files
Output Status File
The output status file, <output_file>.st#, where # is 0-9999, contains the
following runtime reports:
■
Start and end times for each CPU phase.
■
Options settings, with warnings for obsolete options.
■
Status of preprocessing checks for licensing, input syntax, models, and
circuit topology.
■
Convergence strategies that HSPICE uses on difficult circuits.
You can use the information in this file to diagnose problems, particularly when
communicating with Synopsys Customer Support.
Output Tables
The .DCMATCH output tables file, <output_file>.dm#, contains the
variability data from analysis.
Subcircuit Cross-Listing File
If the input netlist includes subcircuits, HSPICE automatically generates a
subcircuit cross-listing file, <output_file>.pa#, where # is 0-9999. This
file relates the subcircuit node names, in the subcircuit call, to the node names
used in the corresponding subcircuit definitions. In HSPICE RF, you cannot
replicate output commands within subcircuit (subckt) definitions.
Transient Analysis Measurement Results File
HSPICE writes transient analysis measurement results to file
<output_file>.mt# when the input file includes an .MEASURE TRAN
statement.
Transient Analysis Results File
Both HSPICE and HSPICE RF place the results of transient analysis in file
<output_file>.tr#, where # is 0-9999, as set forth in the -n commandline argument. This file lists the numerical results of transient analysis.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
19
Chapter 2: Setup and Simulation
Running HSPICE Simulations
A .TRAN statement in the input file, together with an .OPTION POST
statement, creates this post-analysis file.
If the input file includes an .OPTION POST statement, then the output file
contains simulation output suitable for a waveform display tool.
Running HSPICE Simulations
Use the following syntax to start HSPICE:
hspice <-i <path/input_file>> <-o <path/output_file>>
<-n number> <-html <path/html_file>> <-b> <-d>
<-C <path/input_file>> <-I> <-K> <-L command_file>
<-S> <-mt number> <-meas measurefile> <-hdl filename>
<-hdlpath pathname> <<name> -vamodel <name2>...>
For a description of the hspice command syntax and arguments, see
“HSPICE Command Syntax” in the HSPICE Command Reference.
When your invoke an HSPICE simulation, the following sequence of events
occurs:
1. Invocation.
For example, at the shell prompt, enter:
hspice demo.sp > demo.out &
This command invokes the UNIX hspice shell command on input netlist file
demo.sp and directs the output listing to file demo.out. The “&” character at
the end of the command invokes HSPICE in the background, so that you can
continue to use the window and keyboard while HSPICE runs.
2. Script execution.
The hspice shell command starts the HSPICE executable from the
appropriate architecture (machine type) directory. The UNIX run script
launches a HSPICE simulation. This procedure establishes the environment
for the HSPICE executable. The script prompts for information, such as the
platform that you are using, and the version of HSPICE to run. (Available
versions are determined when you install HSPICE.)
3. Licensing.
HSPICE supports the FLEXlm licensing management system. When you
use FLEXlm licensing, HSPICE reads the LM_LICENSE_FILE environment
variable to find the location of the license.dat file.
20
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Running HSPICE Simulations
If HSPICE cannot authorize access, the job terminates at this point, and
prints an error message in the output listing file.
4. Simulation configuration.
HSPICE reads the appropriate meta.cfg file. The search order for the
configuration file is the user login directory, and then the product installation
directory.
5. Design input.
HSPICE opens the input netlist file demo.sp. If this file does not exist, a no
input data error appears in the output listing file.
(UNIX) HSPICE opens three scratch files in the /tmp directory. To change
this directory, reset the tmpdir environment variable in the HSPICE
command script.
(Windows) HSPICE opens three scratch files in the c:\<path>\TEMP (or
\TMP) directory. To change this directory, reset the TEMP or TMP
environment variable in the HSPICE command script.
HSPICE opens the output listing file demo.out for writing. If you do not own
the current directory, HSPICE terminates with a file open error.
Here’s an example of a simple HSPICE input netlist:
Inverter Circuit
.OPTION LIST NODE POST
.TRAN 200P 20N SWEEP TEMP -55 75 10
.PRINT TRAN V(IN) V(OUT)
M1 VCC IN OUT VCC PCH L=1U W=20U
M2 OUT IN 0 0 NCH L=1U W=20U
VCC VCC 0 5
VIN IN 0 0 PULSE .2 4.8 2N 1N 1N 5N 20N
CLOAD OUT 0 .75P
.MODEL PCH PMOS
.MODEL NCH NMOS
.ALTER
CLOAD OUT 0 1.5P
.END
6. Library input.
HSPICE reads any files that you specified in .INCLUDE and .LIB
statements.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
21
Chapter 2: Setup and Simulation
Running HSPICE RF Simulations
7. Operating point initialization.
HSPICE reads any initial conditions that you specified in .IC and
.NODESET statements, finds an operating point (that you can save with
a .SAVE statement), and writes any operating point information that you
requested.
8. Multipoint analysis.
HSPICE performs the experiments specified in analysis statements. In the
above example, the .TRAN statement causes HSPICE to perform a
multipoint transient analysis for 20 ns for temperatures ranging from -55°C
to 75°C, in steps of 10°C.
9. Single-point analysis.
HSPICE performs a single or double sweep of the designated quantity, and
produces one set of output files.
10. Worst-case .ALTER.
You can vary simulation conditions, and repeat the specified single or
multipoint analysis. The above example changes CLOAD from 0.75 pF to 1.5
pF, and repeats the multipoint transient analysis.
11. Normal termination.
After you complete the simulation, HSPICE closes all files it opened and
releases all license tokens.
Running HSPICE RF Simulations
Use the following syntax to invoke HSPICE RF:
hspicerf [-a] inputfile [outputfile] [-h] [-v]
For a description of the hspicerf command syntax and arguments, see
“HSPICE RF Command Syntax” in the HSPICE Command Reference.
22
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Running HSPICE Interactively
Running HSPICE Interactively
When HSPICE is in the interactive mode, you can then use these HSPICE
commands at the HSPICE prompt to help you simulate circuits interactively:
ac [...statement]
cd
dc [...statement]
edit
help
info outflag
input
list [lineno]
load filename
ls [directory]
measure [statement]
op
print <tran/ac/dc>,v/vm/vr/vi/vp/vdb>
pwd
quit
run
save <netlist/command> filename
set outflag <true/false>
tran [...statement]
To Start Interactive Mode
Starting HSPICE in the interactive mode lets you use a subset of commands to
simulate your circuits interactively. To invoke the interactive mode, enter:
hspice -I
You can also use the help command at the HSPICE prompt for an annotated
list of the commands supported in the interactive mode.
The interactive mode also supports saving commands into a script file. To save
the commands that you use, and replay them later, enter:
HSPICE > save command <filename>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
23
Chapter 2: Setup and Simulation
Running Multithreading HSPICE Simulations
To Run a Command File in Interactive Mode
To run the command you have saved in a command file, enter:
hspice -I -L <filename>
To Quit Interactive Mode
To exit the interactive mode and return to the system prompt, enter:
HSPICE > quit
Running Multithreading HSPICE Simulations
HSPICE simulations include device model evaluations and matrix solutions.
You can run model evaluations concurrently on multiple CPUs, by using
multithreading to significantly improve simulation performance. Model
evaluation dominates most of the time. To determine how much time HSPICE
spends evaluating models and solving matrices, specify .OPTION ACCT=2 in
the netlist.
By using multithreading, you can speed-up simulations with no loss of
accuracy. Multithreading gives the best results for circuit designs that contain
many MOSFET, JFET, diode, or BJT models in the netlist.
To Run Multithreading
To run multithreading on UNIX platforms, enter:
hspice -mt number -i <input_file> -o <output_file>
To run multithreading on Windows platforms, enter:
hspice_mt.exe -mt number -i <input_file> -o <output_file>
■
If you omit the number parameter, an error message results. You must
include this parameter.
■
If you specify a number parameter that is larger than the number of available
CPUs, then HSPICE sets the number of threads equal to the number of
available CPUs.
For additional information about command-line options, see “HSPICE
Command Syntax” in the HSPICE Command Reference.
24
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Running Multithreading HSPICE Simulations
In Windows NT Explorer:
1. Double-click the hsp_mt application icon.
2. Select the File/Simulate button, to select the input netlist file.
In Windows, the program automatically detects the number of available
processors.
Under the Synopsys HSPICE User Interface (HSPUI):
1. Select the correct hsp_mt.exe version in the Version combo box.
2. Select the correct number of CPUs in the MT option box.
3. Click the Open button to select the input netlist file.
4. Click the Simulate button to start the simulation.
Performance Improvement Estimations
For HSPICE-MT, the CPU time is:
Tmt=Tserial + Tparallel/Ncpu + Toverhead
Where:
Tserial represents HSPICE calculations that are not threaded.
Tparallel represents threaded HSPICE calculations.
Ncpu is the number of CPUs used.
Toverhead is the overhead from multithreading. Typically, this represents a
small fraction of the total runtime.
For example, for a 151-stage NAND ring oscillator using LEVEL 49,
Tparallel is about 80% of T1cpu (the CPU time associated with a single
CPU) if you run with two threads on a multi-CPU ma
HSPICE® Simulation and Analysis User Guide
Y-2006.03
25
Chapter 2: Setup and Simulation
Using HSPICE in Client/Server Mode
Using HSPICE in Client/Server Mode
When you run many small simulation cases, you can use the client/server
mode to improve performance. This performance improvement occurs because
you check out and check in an HSPICE license only once. This is an effective
measure when you characterize cells.
To Start Client/Server Mode
Starting the client/server mode creates an HSPICE server and checks out an
HSPICE license. To start the client/server mode, enter:
hspice -C
Server
The server name is a specific name connected with the machine on which
HSPICE runs. When you create the server, HSPICE also generates a
hidden .hspicecc directory in your home directory. HSPICE places some
related files in this directory, and removes them when the server exits.
HSPICE Client/Server mode does not let one user create several servers on
the same machine.
When you create a server, the output on the screen is:
***************************************
*Starting HSPICE Client/Server Mode...*
***************************************
Checking out HSPICE license...
HSPICE license has been checked out.
***********************************************
*Welcome to HSPICE Client/Server Mode!*
*******************************************
After you create the server, it automatically runs in the background.
If the server does not receive any request from a client for 12 hours, the server
releases the license, and exits automatically.
26
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 2: Setup and Simulation
Using HSPICE in Client/Server Mode
Client
The client can send a request to the server to ask whether an HSPICE license
has been checked out, or to kill the server.
■
If the request is to check the license status, the server checks whether an
HSPICE license has been checked out, and replies to the client. The syntax
of this request is:
hspice -C casename.sp
Where casename is the name of the circuit design to simulate.
■
If the client receives ok, it begins to simulate the circuit design.
■
If the client receives no, it exits.
■
If the server receives several requests at the same time, it queues these
requests, and process them in the order that the server received them.
■
If HSPICE does not find a server, it creates a server first. Then the server
checks out an HSPICE license, and simulates the circuit.
■
If the request is to kill the server, the server releases the HSPICE license
and other sources, and exits.
When you kill the server, any simulation cases that are queued on that
server do not run, and the server's name disappears from the
hidden .hspicecc directory in your home directory.
If you do not specify an output file, HSPICE directs output to the client terminal.
Use the following syntax to redirect the output to a file, instead of to the
terminal:
hspice -C casename.sp > <output_file>
Note:
HSPICE RF does not support PKG and EBD simulation.
To Simulate a Netlist in Client/Server Mode
Once you have started the client/server mode, which automatically checks out
an HSPICE license, you can run simulations. To simulate a netlist in
client/server mode, enter:
hspice -C <path/input_file>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
27
Chapter 2: Setup and Simulation
Running HSPICE to Calculate New Measurements
Note:
This mode also supports other HSPICE command line options. For a
description of the options shown, see “HSPICE Command Syntax” in the
HSPICE Command Reference.
To Quit Client/Server Mode
Quitting the client/server mode releases the HSPICE license and exits
HSPICE. To exit the client/server mode, enter:
hspice -C -K
Running HSPICE to Calculate New Measurements
When you want to calculate new measurements from previous simulation
results produced by HSPICE, you can rerun HSPICE.
To Calculate New Measurements
To get new measurements from a previous simulation, enter:
hspice -meas measurefile -i <wavefile> <-o <outputfile>>
For a description of the options shown, see “HSPICE Command Syntax” in the
HSPICE Command Reference.
28
HSPICE® Simulation and Analysis User Guide
Y-2006.03
3
3
Input Netlist and Data Entry
Describes the input netlist file and methods of entering data.
For descriptions of individual HSPICE commands referenced in this chapter,
see the “Netlist Commands” chapter in the HSPICE Command Reference.
Input Netlist File Guidelines
HSPICE and HSPICE RF operate on an input netlist file, and store results in
either an output listing file or a graph data file. An input file, with the name
<design>.sp, contains the following:
■
Design netlist (subcircuits, macros, power supplies, and so on).
■
Statement naming the library to use (optional).
■
Specifies the type of analysis to run (optional).
■
Specifies the type of output desired (optional).
An input filename can be up to 1024 characters long. The input netlist file
cannot be in a packed or compressed format.
To generate input netlist and library input files, HSPICE or HSPICE RF uses
either a schematic netlister or a text editor.
Statements in the input netlist file can be in any order, except that the first line is
a title line, and the last .ALTER submodule must appear at the end of the file
and before the .END statement.
Note:
If you do not place an .END statement and a [Return] at the end of the
input netlist file, HSPICE or HSPICE RF issues an error message.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
29
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
Netlist input processing is case insensitive, except for file names and their
paths. HSPICE and HSPICE RF do not limit the identifier length, line length, or
file size.
Input Line Format
■
The input reader can accept an input token, such as:
•
a statement name.
•
a node name.
•
a parameter name or value.
Any valid string of characters between two token delimiters is a token.
You can use a character string as a parameter value in HSPICE, but not
in HSPICE RF. See Delimiters on page 32.
30
■
An input statement, or equation can be up to 1024 characters long.
■
HSPICE or HSPICE RF ignores differences between upper and lower case
in input lines, except in quoted filenames.
■
To continue a statement on the next line, enter a plus (+) sign as the first
non-numeric, non-blank character in the next line.
■
To indicate “to the power of” in your netlist, use two asterisks (**). For
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
•
Names are input tokens. Token delimiters must precede and follow
names. See “Delimiters” below.
•
Names can be up to 1024 characters long and are not case-sensitive.
•
Do not use any of the time keywords as a parameter name or node
name in your netlist.
•
The following symbols are reserved operator keywords: , () = “ ‘
Do not use these symbols as part of any parameter or node name that
you define. Using any of these reserved operator keywords as names
causes a syntax error, and HSPICE or HSPICE RF stops immediately.
First Character
The first character in every line specifies how HSPICE and HSPICE RF
interprets the remaining line. Table 3lists and describes the valid characters.
Table 3
First Character Descriptions
Line
If the First Character is...
Indicates
First line of a netlist
Any character
Title or comment line. The first
line of an included file is a
normal line and not a
comment.
Subsequent lines of
netlist, and all lines of
included files
. (period)
Netlist keyword. For example,
.TRAN 0.5ns 20ns
c, C, d, D, e, E, f, F, g, G, h,
H, i, I, j, J, k, K, l, L, m, M,
q, Q, r, R, s, S, v, V,w,W
Element instantiation
* (asterisk)
# (number)
Comment line (HSPICE)
Comment line (HSPICE RF)
+ (plus)
Continues previous line
HSPICE® Simulation and Analysis User Guide
Y-2006.03
31
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
Delimiters
■
An input token is any item in the input file that HSPICE or HSPICE RF
recognizes. Input token delimiters are: tab, blank, comma (,), equal sign (=),
and parentheses ( ).
■
Single (‘) or double quotes (“) delimit expressions and filenames.
■
Colons (:) delimit element attributes (for example, M1:VGS).
■
Periods (.) indicate hierarchy. For example, X1.X2.n1 is the n1 node on the
X2 subcircuit of the X1 circuit.
Node Identifiers
Node identifiers can be up to 1024 characters long, including periods and
extensions. Node identifiers are used for node numbers and node names.
■
Node numbers are valid in the range of 0 through 9999999999999999
(1-1e16).
■
Leading zeros in node numbers are ignored.
■
Trailing characters in node numbers are ignored. For example, node 1A is
the same as node 1.
■
A node name can begin with any of these characters:
! # % * / < > _ ? | . &
For additional information, see Node Naming Conventions on page 44.
■
To make node names global across all subcircuits, use a .GLOBAL
statement.
■
The 0, GND, GND!, and GROUND node names all refer to the global HSPICE
or HSPICE RF ground. Simulation treats nodes with any of these names as
a ground node, and produces v(0) into the output files.
Instance Names
The names of element instances begin with the element key letter (see
Table 4), except in subcircuits where instance names begin with X. (Subcircuits
are sometimes called macros or modules.) Instance names can be up to 1024
32
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
characters long. The .OPTION LENNAM defines the length of names in
printouts (default=8).
Table 4
Element Identifiers
Letter
(First
Char)
Element
Example Line
B
IBIS buffer
b_io_0 nd_pu0 nd_pd0
nd_out nd_in0 nd_en0
nd_outofin0 nd_pc0 nd_gc0
C
Capacitor
Cbypass 1 0 10pf
D
Diode
D7 3 9 D1
E
Voltage-controlled voltage source
Ea 1 2 3 4 K
F
Current-controlled current source
Fsub n1 n2 vin 2.0
G
Voltage-controlled current source
G12 4 0 3 0 10
H
Current-controlled voltage source
H3 4 5 Vout 2.0
I
Current source
I A 2 6 1e-6
J
JFET or MESFET
J1 7 2 3 GAASFET
K
Linear mutual inductor (general form) K1 L1 L2 1
L
Linear inductor
LX a b 1e-9
M
MOS transistor
M834 1 2 3 4 N1
P
Port
P1 in gnd port=1 z0=50
Q
Bipolar transistor
Q5 3 6 7 8 pnp1
R
Resistor
R10 21 10 1000
S, T, U,
W
Transmission line
S1 nd1 nd2 s_model2
V
Voltage source
V1 8 0 5
HSPICE® Simulation and Analysis User Guide
Y-2006.03
33
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
Table 4
Element Identifiers (Continued)
Letter
(First
Char)
Element
Example Line
W
Transmission Line
W1 in1 0 out1 0 N=1 L=1
X
Subcircuit call
X1 2 4 17 31 MULTI WN=100
LN=5
Hierarchy Paths
■
A period (.) indicates path hierarchy.
■
Paths can be up to 1024 characters long.
■
Path numbers compress the hierarchy for post-processing and listing files.
■
You can find path number cross references in the listing and in the
<design>.pa0 file.
■
The .OPTION PATHNUM controls whether the list files show full path names
or path numbers.
Numbers
You can enter numbers as integer, floating point, floating point with an integer
exponent, or integer or floating point with one of the scale factors listed in
Table 5.
Table 5
34
Scale Factors
Scale Factor
Prefix
Symbol
Multiplying Factor
T
tera
T
1e+12
G
giga
G
1e+9
MEG or X
mega
M
1e+6
K
kilo
k
1e+3
M
milli
m
1e-3
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
Table 5
Scale Factors (Continued)
Scale Factor
Prefix
Symbol
Multiplying Factor
U
micro
μ
1e-6
N
nano
n
1e-9
P
pico
p
1e-12
F
femto
f
1e-15
A
atto
a
1e-18
Note:
Scale factor A is not a scale factor in a character string that contains amps.
For example, HSPICE interprets the 20amps string as 20e-18mps (2018mps), but it correctly interprets 20amps as 20 amperes of current, not as
20e-18mps (20-18mps).
■
Numbers can use exponential format or engineering key letter format, but
not both (1e-12 or 1p, but not 1e-6u).
■
To designate exponents, use D or E.
■
The .OPTION EXPMAX limits the exponent size.
■
Trailing alphabetic characters are interpreted as units comments.
■
Units comments are not checked.
■
The .OPTION INGOLD controls the format of numbers in printouts.
■
The .OPTION NUMDGT=x controls the listing printout accuracy.
■
The .OPTION MEASDGT=x controls the measure file printout accuracy.
■
The .OPTION VFLOOR=x specifies the smallest voltage for which HSPICE
or HSPICE RF prints the value. Smaller voltages print as 0.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
35
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
Parameters and Expressions
■
Parameter names in HSPICE or HSPICE RF use HSPICE name syntax
rules, except that names must begin with an alphabetic character. The other
characters must be either a number, or one of these characters:
! # $ % [ ] _
■
To define parameter hierarchy overrides and defaults, use the .OPTION
PARHIER=global | local statement.
■
If you create multiple definitions for the same parameter or option, HSPICE
or HSPICE RF uses the last parameter definition or .OPTION statement,
even if that definition occurs later in the input than a reference to the
parameter or option. HSPICE or HSPICE RF does not warn you when you
redefine a parameter.
■
You must define a parameter before you use that parameter to define
another parameter.
■
When you select design parameter names, be careful to avoid conflicts with
parameterized libraries.
■
To delimit expressions, use single or double quotes.
■
Expressions cannot exceed 1024 characters.
■
For improved readability, use a double slash (\\) at end of a line, to continue
the line.
■
You can nest functions up to three levels.
■
Any function that you define can contain up to two arguments.
■
Use the PAR (expression or parameter) function to evaluate expressions in
output statements.
Input Netlist File Structure
An input netlist file should consist of one main program, and one or more
optional submodules. Use a submodule (preceded by an .ALTER statement) to
automatically change an input netlist file; then rerun the simulation with
different options, netlist, analysis statements, and test vectors.
You can use several high-level call statements (.INCLUDE, .LIB and .DEL
LIB) to restructure the input netlist file modules. These statements can call
netlists, model parameters, test vectors, analysis, and option macros into a file,
36
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
from library files or other files. The input netlist file also can call an external data
file, which contains parameterized data for element sources and models. You
must enclose the names of included or internally-specified files in single or
double quotation when they begin with a number (0-9).
Schematic Netlists
HSPICE or HSPICE RF typically use netlisters to generate circuits from
schematics, and accept either hierarchical or flat netlists.
The process of creating a schematic involves:
■
Symbol creation with a symbol editor.
■
Circuit encapsulation.
■
Property creation.
■
Symbol placement.
■
Symbol property definition.
■
Wire routing and definition
Table 6
Input Netlist File Sections
Sections
Examples
Definition
Title
.TITLE
The first line in the netlist is the title of the
input netlist file.
Set-up
.OPTION .IC or .NODESET,
.PARAM, .GLOBAL
Sets conditions for simulation.
Initial values in circuit and subcircuit.
Set parameter values in the netlist.
Set node name globally in netlist.
Sources
Sources and digital inputs
Sets input stimuli (I or V element).
Netlist
Circuit elements
.SUBKCT, .ENDS, or
.MACRO, .EOM
Circuit for simulation.
Subcircuit definitions.
Analysis
.DC, .TRAN, .AC, and so on.
.SAVE and .LOAD
.DATA, .TEMP
Statements to perform analyses.
Save and load operating point information.
Create table for data-driven analysis.
Set temperature analysis.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
37
Chapter 3: Input Netlist and Data Entry
Input Netlist File Guidelines
Table 6
Input Netlist File Sections (Continued)
Sections
Examples
Definition
Output
.PRINT, .PLOT, .GRAPH,
.PROBE, .MEASURE
Statements to output variables.
Statement to evaluate and report userdefined functions of a circuit.
Library,
Model and
File
Inclusion
.INCLUDE
General include files.
.MALIAS
Assigns an alias to a diode, BJT, JFET, or
MOSFET.
.MODEL
Element model descriptions.
.LIB
Library.
.OPTION SEARCH
Search path for libraries and included files.
.PROTECT and .UNPROTECT
Control printback to output listing.
Alter blocks
.ALIAS, .ALTER, .DEL LIB
Renames a previous model.
Sequence for in-line case analysis.
Removes previous library selection.
End of
netlist
.END
Required statement; end of netlist.
38
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Input Netlist File Composition
The HSPICE and HSPICE RF circuit description syntax is compatible with the
SPICE input netlist format. Figure 7 shows the basic structure of an input
netlist.
Figure 7
Basic Netlist Structure
Title line: First line is automatically a comment
* Comments (all lines beginning with an asterisk)
*
Input control statements
Netlist body: description of circuit topology.
.MODEL statements
*
.OPTION statements
.OPTION with option statements
.PRINT and other output statements.
Analysis statement (such as .POWER, .TRAN)
.END
Element and input
control statements
Analysis/output
control statements
The following is an example of a simple netlist file, called inv_ckt.in. It shows a
small inverter test case that measures the timing behavior of the inverter.
To create the circuit:
1. Define the MOSFET models for the PMOS and NMOS transistors of the
inverter.
2. Insert the power supplies for both VDD and GND power rails.
Insert the pulse source to the inverter input.
This circuit uses transient analysis and produces output graphical waveform
data for the input and output ports of the inverter circuit.
* Sample inverter circuit
* **** MOS models *****
.MODEL n1 NMOS LEVEL=3 THETA=0.4 ...
.MODEL p1 PMOS LEVEL=3 ...
* ***** Define power supplies and sources *****
VDD VDD 0 5
VPULSE VIN 0 PULSE 0 5 2N 2N 2N 98N 200N
VGND GND 0 0
* ***** Actual circuit topology *****
M1 VOUT VIN VDD VDD p1
M2 VOUT VIN GND GND n1
* ***** Analysis statement *****
HSPICE® Simulation and Analysis User Guide
Y-2006.03
39
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
.TRAN 1n 300n
* ***** Output control statements *****
.OPTION POST PROBE
.PROBE V(VIN) V(VOUT)
.END
For a description of individual commands used in HSPICE or HSPICE RF
netlists, see the “Netlist Commands” chapter in the HSPICE Command
Reference.
Title of Simulation
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.
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 use the .TITLE statement. To change
a title for a .ALTER statement, place the title content in the .ALTER statement
itself.
Comments and Line Continuation
The first line of a netlist is always a comment, regardless of its first character;
comments that are not the first line of the netlist require either an asterisk (*) in
HSPICE or a number sign (#) in HSPICE RF as the first character of the line, or
a dollar sign ($) directly in front of the comment anywhere on the line. For
example,
* <comment_on_a_line_by_itself>
-or<HSPICE_statement> $ <comment_following_HSPICE_input>
You can place comment statements anywhere in the circuit description.
40
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
The dollar sign must be used for comments that do not begin in the first
character position on a line (for example, for comments that follow simulator
input on the same line). If it is not the first nonblank character, then the dollar
sign must be preceded by either:
■
Whitespace
■
Comma (,)
■
Valid numeric expression.
You can also place the dollar sign within node or element names. For example,
* RF=1K GAIN SHOULD BE 100
$ MAY THE FORCE BE WITH MY CIRCUIT
VIN 1 0 PL 0 0 5V 5NS $ 10v 50ns
R12 1 0 1MEG $ FEED BACK
.PARAM a=1w$comment a=1, w treated as a space and ignored
.PARAM a=1k$comment a=1e3, k is a scale factor
A dollar sign is the preferred way to indicate comments, because of the
flexibility of its placement within the code.
Line continuations require a plus sign (+) as the first character in the line that
follows. Here is an example of comments and line continuation in a netlist file:
.ABC Title Line (HSPICE or HSPICE RF ignores the netlist keyword
* on this line, because the first line is always a comment)
* This is a comment line
.MODEL n1 NMOS $ this is an example of an inline comment
* This is a comment line and the following line is a continuation
+ LEVEL=3
Element and Source Statements
Element statements describe the netlists of devices and sources. Use nodes to
connect elements to one another. Nodes can be either numbers or names.
Element statements specify:
■
Type of device.
■
Nodes to which the device is connected.
■
Operating electrical characteristics of the device.
Element statements can also reference model statements that define the
electrical parameters of the element.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
41
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Table 7 lists the parameters of an element statements.
Table 7
Element Parameters
Parameter
Description
elname
Element name that cannot exceed 1023 characters, and must begin with a
specific letter for each element type:
B IBIS buffer
C Capacitor
D Diode
E,F,G,H Dependent current and voltage sources
I
Current (inductance) source
J JFET or MESFET
K Mutual inductor
L Inductor model or magnetic core mutual inductor model
M MOSFET
Q BJT
P Port
R Resistor
S, T, U, WTransmission line
V Voltage source
X Subcircuit call
node1 ...
Node names identify the nodes that connect to the element. The node name
begins with a letter and can contain a maximum of 1023 characters. You cannot
use the following characters in node names:=( ),’ <space>
mname
HSPICE or HSPICE RF requires a model reference name for all elements, except
passive devices.
pname1 ...
An element parameter name identifies the parameter value that follows this
name.
expression
Any mathematical expression containing values or parameters, such as
param1 * val2
val1 ...
Value of the pname1 parameter, or of the corresponding model node. The value
can be a number or an algebraic expression.
M=val
Element multiplier. Replicates val element times, in parallel. Do not assign a
negative value or zero as the M value.
42
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
For descriptions of element statements for the various types of supported
elements, see the chapters about individual types of elements in this user
guide.
Example 1
Q1234567
4000
5000 6000 SUBSTRATE BJTMODEL AREA=1.0
The preceding example specifies a bipolar junction transistor, with its collector
connected to node 4000, its base connected to node 5000, its emitter
connected to node 6000, and its substrate connected to the SUBSTRATE node.
The BJTMODEL name references the model statement, which describes the
transistor parameters.
M1 ADDR SIG1 GND SBS N1 10U 100U
The preceding example specifies a MOSFET named M1, where:
■
drain node=ADDR
■
gate node=SIG1
■
source node=GND
■
substrate nodes=SBS
The preceding element statement calls an associated model statement, N1.
The MOSFET dimensions are width=100 microns and length=10 microns.
Example 2
M1 ADDR SIG1 GND SBS N1 w1+w l1+l
The preceding example specifies a MOSFET named M1, where:
■
drain node=ADDR
■
gate node=SIG1
■
source node=GND
■
substrate nodes=SBS
The preceding element statement calls an associated model statement, N1.
MOSFET dimensions are algebraic expressions (width=w1+w, and
length=l1+l).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
43
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Defining Subcircuits
You can create a subcircuit description for a commonly-used circuit, and
include one or more references to the subcircuit in your netlist.
■
Use .SUBCKT and .MACRO statements to define subcircuits within your
HSPICE netlist or HSPICE RF.
■
Use the .ENDS statement to terminate a .SUBCKT statement.
■
Use the .EOM statement to terminate a .MACRO statement.
■
Use X<subcircuit_name> (the subcircuit call statement) to call a
subcircuit that you previously defined in a .MACRO or .SUBCKT command in
your netlist, where <subcircuit_name> is the element name of the subcircuit
that you are calling. This subcircuit element name can be up to 15
characters long.
■
Use the .INCLUDE statement to include another netlist as a subcircuit in the
current netlist.
Node Naming Conventions
Nodes are the points of connection between elements in the input netlist. You
can use either names or numbers to designate nodes. Node numbers can be
from 1 to 999999999999999; node number 0 is always ground. HSPICE or
HSPICE RF ignores letters that follow numbers in node names. When the node
name begins with a letter or a valid special character, the node name can
contain a maximum of 1024 characters.
In addition to letters and digits, node names can include the following
characters:
+, -, *, /, $, #, [], !, <>, _, %
Node names that begin with one or more numerical digits cannot contain
brackets; for example, 123[r55]. Whereas, node names that begin with
alphabetic character may contain brackets; for example, n123[r55].
If you use braces { } in node names, HSPICE or HSPICE RF changes them to
brackets [ ].
You cannot use the following characters in node names: () ,=‘ <blank>
You should avoid using the dollar sign ($) after a numerical digit in a node
name, because HSPICE assumes whatever follows the "$" symbol is an in-line
comment (see Comments and Line Continuation on page 40 for additional
44
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
information). It can cause error and warning messages depending on where
the node containing the "$" is located. For example, HSPICE generates an
error indicating that a resistor node is missing:
R1 1$ 2 1k
Also, in this example, HSPICE issues a warning indicating that the value of
resistor R1 is limited to 1e-5 and interprets the line as “R1 2 1“ without a
defined value:
R1 2 1$ 1k
The period (.) is reserved for use as a separator between a subcircuit name
and a node name: subcircuitName.nodeName. If a node name contains a
period, the node will be considered a top level node unless there is a valid
match to a subcircuit name and node name in the hierarchy.
The sorting order for operating point nodes is:
a-z, !, #, $, %, *, +, -, /
Using Wildcards on Node Names
You can use wildcards to match node names.
■
? wildcard matches any single character. For example, 9? matches 92, 9a,
9A, and 9%.
■
* wildcard matches any string of zero or more characters. For example:
■
•
If your netlist includes a resistor named r1 and a voltage source named
vin, then .PRINT i(*) prints the current for both of these elements:
i(r1) and i(vin).
•
And .PRINT v(o*) prints the voltages for all nodes whose names start
with o; if your netlist contains nodes named in and out, this example
prints only the v(out) voltage.
[ ] matches any character tht appears within the brackets. For example,
[123] matches 1, 2, or 3. A hyphen inside the brackets indicates a
character range. For example, [0-9] is the same as [0123456789], and
matches any digit.
For example, the following prints the results of a transient analysis for the
voltage at the matched node name.
.PRINT TRAN V(9?t*u)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
45
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Wildcards must begin with a letter or a number; for example,
.PROBE v(*)
.PROBE *
.PROBE x*
$ correct format
$ incorrect format
$ correct format
Here are some practical applications for these wildcards:
■
If your netlist includes a resistor named r1 and a voltage source named
vin, then .PRINT i(*) prints the current for both elements i(r1) and
i(vin).
■
The statement .PRINT v(o*) prints the voltages for all nodes whose
names start with o; if your netlist contains nodes named in and out, this
example prints only the v(out) voltage.
■
If your netlist contains nodes named 0, 1, 2, and 3, then .PRINT v(0,*)
or .PRINT v(0 *) prints the voltage between node 0 and each of the other
nodes: v(0,1), v(0,2), and v(0,3).
Examples
The following examples use wildcards with .PRINT, .PROBE, and .LPRINT
statements.
■
Probe node voltages for nodes at all levels.
.PROBE v(*)
■
Probe all nodes whose names start with “a”. For example: a1, a2, a3, a00,
ayz.
.PROBE v(a*)
■
Print node voltages for nodes at the first level and all levels below the first
level, where zero-level are top-level nodes. For example: X1.A, X4.554,
Xab.abc123.
.PRINT v(*.*)
■
Probe node voltages for all nodes whose name start with “x” at the first level
and all levels below the first level, where zero-level are top-level nodes. For
example: x1.A, x4.554, xab.abc123.
.PROBE v(x*.*)
■
Print node voltages for nodes whose names start with “x” at the second-level
and all levels below the second level. For example: x1.x2.a,
xab.xdff.in.
.PRINT v(x*.*.*)
46
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
■
Match all first-level nodes with names that are exactly two characters long.
For example: x1.in, x4.12.
.PRINT v(x*.*.*)
■
In HSPICE RF, print the logic state of all top-level nodes, whose names start
with b. For example: b1, b2, b3, b56, bac.
.LPRINT (1,4) b*
Element, Instance, and Subcircuit Naming Conventions
Instances and subcircuits are elements and as such, follow the naming
conventions for elements.
Element names in HSPICE or HSPICE RF begin with a letter designating the
element type, followed by up to 1023 alphanumeric characters. Element type
letters are R for resistor, C for capacitor, M for a MOSFET device, and so on
(see Element and Source Statements on page 41).
Subcircuit Node Names
HSPICE assigns two subcircuit node names.
■
To assign the first name, HSPICE or HSPICE RF uses the (.) extension to
concatenate the circuit path name with the node name—for example,
X1.XBIAS.M5.
Node designations that start with the same number, followed by any letter,
are the same node. For example, 1c and 1d are the same node.
■
The second subcircuit node name is a unique number that HSPICE
automatically assigns to an input netlist subcircuit. The ( : ) extension
concatenates this number with the internal node name, to form the entire
subcircuit’s node name (for example, 10:M5). The output listing file crossreferences the node name.
Note:
HSPICE RF does not support short names for internal subcircuits, such
as 10:M5.
To indicate the ground node, use either the number 0, the name GND, or !GND.
Every node should have at least two connections, except for transmission line
nodes (unterminated transmission lines are permitted) and MOSFET substrate
HSPICE® Simulation and Analysis User Guide
Y-2006.03
47
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
nodes (which have two internal connections). Floating power supply nodes are
terminated with a 1Megohm resistor and a warning message.
Path Names of Subcircuit Nodes
A path name consists of a sequence of subcircuit names, starting at the
highest-level subcircuit call, and ending at an element or bottom-level node.
Periods separate the subcircuit names in the path name. The maximum length
of the path name, including the node name, is 1024 characters.
You can use path names in .PRINT, .PLOT, .NODESET, and .IC
statements, as another way to reference internal nodes (nodes not appearing
on the parameter list). You can use the path name to reference any node,
including any internal node. Subcircuit node and element names follow the
rules shown in Figure 8 on page 48.
Figure 8
Subcircuit Calling Tree, with Circuit Numbers and Instance Names
0 (CKT)
1 (X1)
3 (X3)
sig24
2 (X2)
n (abc) is
circuit number (instance name)
4 (X4)
sig25
sig26
In Figure 8, the path name of the sig25 node in the X4 subcircuit is
X1.X4.sig25. You can use this path in HSPICE or HSPICE RF statements,
such as:
.PRINT v(X1.X4.sig25)
Abbreviated Subcircuit Node Names
In HSPICE, you can use circuit numbers as an alternative to path names, to
reference nodes or elements in .PRINT, .PLOT, .NODESET, or .IC
48
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
statements. Compiling the circuit assigns a circuit number to all subcircuits,
creating an abbreviated path name:
<subckt-num>:<name>
Note:
HSPICE RF does not recognize this type of abbreviated subcircuit name.
The subcircuit name and a colon precede every occurrence of a node or
element in the output listing file. For example, 4:INTNODE1 is a node named
INTNODE1, in a subcircuit assigned the number 4.
Any node not in a subcircuit has a 0: prefix (0 references the main circuit). To
identify nodes and subcircuits in the output listing file, HSPICE uses a circuit
number that references the subcircuit where the node or element appears.
Abbreviated path names let you use DC operating point node voltage output, as
input in a .NODESET statement for a later run.
You can copy the part of the output listing titled Operating Point Information or
you can type it directly into the input file, preceded by a .NODESET statement.
This eliminates recomputing the DC operating point in the second simulation.
Automatic Node Name Generation
HSPICE or HSPICE RF can automatically assign internal node names. To
check both nodal voltages and branch currents, you can use the assigned node
name when you print or plot. HSPICE or HSPICE RF supports several special
cases for node assignment—for example, simulation automatically assigns
node 0 as a ground node.
For CSOS (CMOS Silicon on Sapphire), if you assign a value of -1 to the bulk
node, the name of the bulk node is B#. Use this name to print the voltage at the
bulk node. When printing or plotting current—for example .PLOT I(R1)—
HSPICE inserts a zero-valued voltage source. This source inserts an extra
node in the circuit named Vnn, where nn is a number that HSPICE (or HSPICE
RF) automatically generates; this number appears in the output listing file.
Global Node Names
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.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
49
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
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.
Circuit Temperature
To specify the circuit temperature for a 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 TNOM control option. 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 .TEMP statements in a circuit behave
as a sweep function.
Data-Driven Analysis
In data-driven analysis, you can modify any number of parameters, then use
the new parameter values to perform an operating point, DC, AC, or transient
analysis. An array of parameter values can be either inline (in the simulation
input file) or stored as an external ASCII file. The .DATA statement associates
a list of parameter names with corresponding values in the array.
HSPICE supports the entire functionality of the .DATA statement. However,
HSPICE RF supports .DATA only for:
■
Data-driven analysis.
■
Inline or external data files.
For more details about using the .DATA statement in different types of analysis,
see Chapter 8, Initializing DC/Operating Point Analysis and Chapter 9,
Transient Analysis.
50
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Library Calls and Definitions
To create and read from libraries of commonly-used commands, device
models, subcircuit analysis, and statements 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.
Library Building Rules
■
A library cannot contain .ALTER statements.
■
A library can contain nested .LIB calls to itself or to other libraries. If you
use a relative path in a nested .LIB call, the path starts from the directory
of the parent library, not from the work directory. If the path starts from the
work directory, HSPICE can also find the library, but it prints a warning. The
depth of nested calls is limited only by the constraints of your system
configuration.
■
A library cannot contain a call to a library of its own entry name, within the
same library file.
■
A HSPICE or HSPICE RF library cannot contain the .END statement.
■
.ALTER processing cannot change .LIB statements, within a file that
an .INCLUDE statement calls.
Automatic Library Selection
Automatic library selection searches a sequence of up to 40 directories. The
hspice.ini file sets the default search paths.
Note:
HSPICE RF does not read the hspice.ini file.
Use this file for directories that you want HSPICE to always search. HSPICE
searches for libraries in the order specified in .OPTION SEARCH statements.
When HSPICE encounters a subcircuit call, the search order is:
1. Read the input file for a .SUBCKT or .MACRO with the specified call name.
2. Read any .INC files or .LIB files for a .SUBCKT or .MACRO with the
specified call name.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
51
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
3. Search the directory containing the input file for the call_name.inc file.
4. Search the directories in the .OPTION SEARCH list.
You can use the HSPICE library search and selection features to simulate
process corner cases, using .OPTION SEARCH =‘<libdir>’ to target
different process directories. For example, if you store an input or output buffer
subcircuit in a file named iobuf.inc, you can create three copies of the file, to
simulate fast, slow and typical corner cases. Each file contains different
HSPICE transistor models, representing the different process corners. Store
these files (all named iobuf.inc) in separate directories.
Defining Parameters
The .PARAM statement defines parameters. Parameters in HSPICE or HSPICE
RF are names that have associated numeric values. You can also use either of
the following specialized methods to define parameters:
■
Predefined Analysis
■
Measurement Parameters
Predefined Analysis
HSPICE or HSPICE RF provides several specialized analysis types, which
require a way to control the analysis. For the syntax used in these .PARAM
commands, see the description of the .PARAM command in the HSPICE
Command Reference.
HSPICE or HSPICE RF supports the following predefined analysis parameters:
■
Temperature functions (fn)
■
Optimization guess/range
HSPICE also supports the following predefined parameter types, that HSPICE
RF does not support:
52
■
frequency
■
time
■
Monte Carlo functions
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Measurement Parameters
A .MEASURE statement produces a measurement parameter. In general, the
rules for measurement parameters are the same as those for standard
parameters. However, measurement parameters are not defined in a .PARAM
statement, but directly in the .MEASURE statement. For more information, see
.MEASURE Parameter Types on page 269.
Altering Design Variables and Subcircuits
The following rules apply when you use an .ALTER block to alter design
variables and subcircuits in HSPICE. This section does not apply to HSPICE
RF.
■
If the name of a new element, .MODEL statement, or subcircuit definition is
identical to the name of an original statement of the same type, then the new
statement replaces the old. Add new statements in the input netlist file.
■
You can alter element and .MODEL statements within a subcircuit definition.
You can also add a new element or .MODEL statement to a subcircuit
definition. To modify the topology in subcircuit definitions, put the element
into libraries. To add a library, use .LIB; to delete, use .DEL LIB.
■
If a parameter name in a new .PARAM statement in the .ALTER module is
identical to a previous parameter name, then the new assigned value
replaces the old value.
■
If you used parameter (variable) values for elements (or model parameter
values) when you used .ALTER, use the .PARAM statement to change
these parameter values. Do not use numerical values to redescribe
elements or model parameters.
■
If you used an .OPTION statement (in an original input file or a .ALTER
block) to turn on an option, you can turn that option off.
■
Each .ALTER simulation run prints only the actual altered input. A
special .ALTER title identifies the run.
■
.ALTER processing cannot revise .LIB statements within a file that
an .INCLUDE statement calls. However, .ALTER processing can
accept .INCLUDE statements, within a file that a .LIB statement calls.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
53
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Using Multiple .ALTER Blocks
This section does not apply to HSPICE RF.
■
For the first simulation run, HSPICE reads the input file, up to the
first .ALTER statement, and performs the analyses up to that .ALTER
statement.
■
After it completes the first simulation, HSPICE reads the input between the
first .ALTER statement, and either the next .ALTER statement or the .END
statement.
■
HSPICE then uses these statements to modify the input netlist file.
■
HSPICE then resimulates the circuit.
■
For each additional .ALTER statement, HSPICE performs the simulation
that precedes the first .ALTER statement.
■
HSPICE then performs another simulation, using the input between the
current .ALTER statement, and either the next .ALTER statement or
the .END statement.
If you do not want to rerun the simulation that precedes the first .ALTER
statement, every time you run an .ALTER simulation, then do the following:
1. Put the statements that precede the first .ALTER statement, into a library.
2. Use the .LIB statement in the main input file.
3. Put a .DEL LIB statement in the .ALTER section, to delete that library for
the .ALTER simulation run.
Connecting Nodes
Use a .CONNECT statement to connect 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. You also cannot use this statement in
HSPICE RF.
54
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
Deleting a Library
Use a .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 a .DEL LIB statement with a .ALTER statement. HSPICE RF
does not support the .ALTER statement.
Ending a Netlist
An .END statement must be the last statement in the input netlist file. Text that
follows the .END statement is a comment, and has no effect on the 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.
Condition-Controlled Netlists (IF-ELSE)
You can use the IF-ELSE structure to change the circuit topology, expand the
circuit, set parameter values for each device instance, select different model
cards, reference subcircuits, or define subcircuits in each IF-ELSE block.
.if (condition1)
<statement_block1>
# The following statement block in {braces} is
# optional, and you can repeat it multiple times:
{ .elseif (condition2)
<statement_block2>
}
# The following statement block in [brackets]
# is optional, and you cannot repeat it:
[ .else
<statement_block3>
]
.endif
HSPICE® Simulation and Analysis User Guide
Y-2006.03
55
Chapter 3: Input Netlist and Data Entry
Input Netlist File Composition
■
In an .IF, .ELSEIF, or .ELSE condition statement, complex Boolean
expressions must not be ambiguous. For example, change (a==b &&
c>=d) to ( (a==b) && (c>=d) ).
■
In an IF, ELSEIF, or ELSE statement block, you can include most valid
HSPICE or HSPICE RF analysis and output statements. The exceptions
are:
•
.END, .ALTER, .GLOBAL, .DEL LIB, .MALIAS, .ALIAS, .LIST,
.NOLIST, and .CONNECT statements.
•
search, d_ibis, d_imic, d_lv56, biasfi, modsrh, cmiflag,
nxx, and brief options.
■
You can include IF-ELSEIF-ELSE statements in subcircuits and subcircuits
in IF-ELSEIF-ELSE statements.
■
You can use IF-ELSEIF-ELSE blocks to select different submodules to
structure the netlist (using .INC, .LIB, and .VEC statements).
■
If two or more models in an IF-ELSE block have the same model name and
model type, they must also be the same revision level.
■
Parameters in an IF-ELSE block do not affect the parameter value within the
condition expression. HSPICE or HSPICE RF updates the parameter value
only after it selects the IF-ELSE block.
■
You can nest IF-ELSE blocks.
■
You can include .SUBCKT and .MACRO statements within an IF-ELSE block.
■
You can include an unlimited number of ELSEIF statements within an
IF-ELSE block.
■
You cannot include sweep parameters or simulation results within an
IF-ELSE block.
■
You cannot use an IF-ELSE block within another statement. In the following
example, HSPICE or HSPICE RF does not recognize the IF-ELSE block as
part of the resistor definition:
r 1 0
.if (r_val>10k)
+ 10k
.else
+ r_val
.endif
56
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Using Subcircuits
Using Subcircuits
Reusable cells are the key to saving labor in any CAD system. This also applies
to circuit simulation, in HSPICE or HSPICE RF.
■
To create and simulate a reusable circuit, construct it as a subcircuit.
■
Use parameters to expand the utility of a subcircuit.
Traditional SPICE includes the basic subcircuit, but does not provide a way to
consistently name nodes. However, HSPICE or HSPICE RF provides a simple
method for naming subcircuit nodes and elements: use the subcircuit call name
as a prefix to the node or element name.
In HSPICE RF, you cannot replicate output commands within subcircuit
(subckt) definitions.
Figure 9
Subcircuit Representation
MP
MN
INV
The following input creates an instance named X1 of the INV cell macro, which
consists of two MOSFETs, named MN and MP:
X1 IN OUT VD_LOCAL VS_LOCAL inv W=20
.MACRO INV IN OUT VDD VSS W=10 L=1 DJUNC=0
MP OUT IN VDD VDD PCH W=W L=L DTEMP=DJUNC
MN OUT IN VSS VSS NCH W=’W/2’ L=L DTEMP=DJUNC
.EOM
Note:
To access the name of the MOSFET, inside of the INV subcircuit that X1
calls, the names are X1.MP and X1.MN. So to print the current that flows
through the MOSFETs, use .PRINT I (X1.MP).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
57
Chapter 3: Input Netlist and Data Entry
Using Subcircuits
Hierarchical Parameters
You can use two hierarchical parameters, the M (multiply) parameter and the S
(scale) parameter.
M (Multiply) Parameter
The most basic HSPICE subcircuit parameter or HSPICE RF is the M (multiply)
parameter. This keyword is common to all elements, including subcircuits,
except for voltage sources. The M parameter multiplies the internal component
values, which in effect creates parallel copies of the element or subcircuit. To
simulate 32 output buffers switching simultaneously, you need to place only one
subcircuit; for example,
X1 in out buffer M=32
Multiply works hierarchically. For a subcircuit within a subcircuit, HSPICE or
HSPICE RF multiplies the product of both levels. Do not assign a negative
value or zero as the M value.
Figure 10
How Hierarchical Multiply Works
X1 in out inv M=2
M=8
mp out in vdd pch W=10 L=1 M=4
M=6
mn out in vss nch W=5 L=1 M=3
UNEXPANDED
58
EXPANDED
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Using Subcircuits
S (Scale) Parameter
To scale a subcircuit, use the S (local scale) parameter. This parameter
behaves in much the same way as the M parameter in the preceding section.
.OPTION hier_scale=value
.OPTION scale=value
X1 node1 node2 subname S=valueM parameter
The OPTION HIER_SCALE statement defines how HSPICE or HSPICE RF
interprets the S parameter, where value is either:
■
0 (the default), indicating a user-defined parameter, or
■
1, indicating a scale parameter.
The .OPTION SCALE statement defines the original (default) scale of the
subcircuit. The specified S scale is relative to this default scale of the subcircuit.
The scale in the subname subcircuit is value*scale. Subcircuits can originate
from multiple sources, so scaling is multiplicative (cumulative) throughout your
design hierarchy.
x1 a y inv S=1u
subckt inv in out
x2 a b kk S=1m
.ends
In this example:
■
HSPICE or HSPICE RF scales the X1 subcircuit by the first S scaling value,
1u*scale.
■
Because scaling is cumulative, X2 (a subcircuit of X1) is then scaled, in
effect, by the S scaling values of both X1 and X2: 1m*1u*scale.
Using Hierarchical Parameters to Simplify Simulation
You can use the hierarchical parameter to simplify simulations. An example is
shown in the following listing and Figure 11 on page 60.
X1 D Q Qbar CL CLBAR dlatch flip=0
.macro dlatch
+ D Q Qbar CL CLBAR flip=vcc
.nodeset v(din)=flip
xinv1 din qbar inv
xinv2 Qbar Q inv
m1 q CLBAR din nch w=5 l=1
m2 D CL din nch w=5 l=1
.eom
HSPICE® Simulation and Analysis User Guide
Y-2006.03
59
Chapter 3: Input Netlist and Data Entry
Subcircuit Call Statement Discrete Device Libraries
Figure 11
D Latch with Nodeset
Q
clbar
cl
Q
D
din
.Nodeset
HSPICE does not limit the size or complexity of subcircuits; they can contain
subcircuit references, and any model or element statement. However, in
HSPICE RF, you cannot replicate output commands within subcircuit
definitions. To specify subcircuit nodes in .PRINT or .PLOT statements,
specify the full subcircuit path and node name.
Undefined Subcircuit Search
(HSPICE) If a subcircuit call is in a data file that does not describe the
subcircuit, HSPICE automatically searches directories in the following order:
1. Present directory for the file.
2. Directories specified in .OPTION SEARCH = “directory_path_name”
statements.
3. Directory where the Discrete Device Library is located.
HSPICE searches for the model reference name file that has an .inc suffix. For
example, if the data file includes an undefined subcircuit, such as
X 1 1 2 INV, HSPICE searches the system directories for the inv.inc file and
when found, places that file in the calling data file.
Subcircuit Call Statement Discrete Device Libraries
The Synopsys Discrete Device Library (DDL) is a collection of HSPICE device
models of discrete components, which you can use with HSPICE or HSPICE
RF. The $<installdir>/parts directory contains the various subdirectories that
form the DDL. Synopsys used its own ATEM discrete device characterization
system to derive the BJT, MESFET, JFET, MOSFET, and diode models from
60
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Subcircuit Call Statement Discrete Device Libraries
laboratory measurements. The behavior of op-amp, timer, comparator, SCR,
and converter models closely resembles that described in manufacturers’ data
sheets. HSPICE and HSPICE RF have a built-in op-amp model generator.
Note:
The value of the $INSTALLDIR environment variable is the pathname to the
directory where you installed HSPICE or HSPICE RF. This installation
directory contains subdirectories, such as /parts and /bin. It also contains
certain files, such as a prototype meta.cfg file, and the license files.
DDL Library Access
To include a DDL library component in a data file, use the X subcircuit call
statement with the DDL element call. The DDL element statement includes the
model name, which the actual DDL library file uses.
For example, the following element statement creates an instance of the
1N4004 diode model:
X1 2 1 D1N4004
Where D1N4004 is the model name.
See Element and Source Statements on page 41 and the HSPICE Elements
and Device Models Manual for descriptions of element statements.
Optional parameter fields in the element statement can override the internal
specification of the model. For example, for op-amp devices, you can override
the offset voltage, and the gain and offset current. Because the DDL library
devices are based on HSPICE circuit-level models, simulation automatically
compensates for the effects of supply voltage, loading, and temperature.
HSPICE or HSPICE RF accesses DDL models in several ways:
■
The installation script creates an hspice.ini initialization file.
■
HSPICE or HSPICE RF writes the search path for the DDL and vendor
libraries into a .OPTION SEARCH=‘<lib_path>’ statement.
This provides immediate access to all libraries for all users. It also
automatically includes the models in the input netlist. If the input netlist
references a model or subcircuit, HSPICE or HSPICE RF searches the
directory to which the DDLPATH environment variable points for a file with
the same name as the reference name. This file is an include file so its
filename suffix is .inc. HSPICE installation sets the DDLPATH variable in the
meta.cfg configuration file.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
61
Chapter 3: Input Netlist and Data Entry
Subcircuit Call Statement Discrete Device Libraries
■
Set .OPTION SEARCH=‘<lib_path>’ in the input netlist.
Use this method to list the personal libraries to search. HSPICE or HSPICE
RF first searches the default libraries referenced in the hspice.ini file, then
searches libraries in the order listed in the input file.
■
Directly include a specific model, using the .INCLUDE statement. For
example, to use a model named T2N2211, store the model in a file named
T2N2211.inc, and put the following statement in the input file:
.INCLUDE <path>/T2N2211.inc
This method requires you to store each model in its own .inc file, so it is not
generally useful. However, you can use it to debug new models, when you
test only a small number of models.
Vendor Libraries
The vendor library is the interface between commercial parts and circuit or
system simulation.
■
ASIC vendors provide comprehensive cells, corresponding to inverters,
gates, latches, and output buffers.
■
Memory and microprocessor vendors supply input and output buffers.
■
Interface vendors supply complete cells for simple functions and output
buffers, to use in generic family output.
■
Analog vendors supply behavioral models.
To avoid name and parameter conflicts, models in vendor cell libraries should
be within the subcircuit definitions.
62
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 3: Input Netlist and Data Entry
Subcircuit Call Statement Discrete Device Libraries
Figure 12
Vendor Library Usage
/usr/lib/vendor/buffer_f.inc
/usr/lib/vendor/skew.dat
.macro buffer_f in out vdd vss
.lib ‘/usr/lib/vendor/skew.dat’ ff
.lib ff $ fast model
.param vendor_xl=-.1u
.inc ‘/usr/lib/vendor/model.dat’
.endl ff
.inc ‘/usr/lib/vendor/buffer.inc’
.eom
Subcircuit Library Structure
Your library structure must adhere to the .INCLUDE statement specification in
the implicit subcircuit. You can use this statement to specify the directory that
contains the <subname>.inc subcircuit file, and then reference the <subname>
in each subcircuit call.
The component naming conventions for each subcircuit is:
<subname>.inc
Store the subcircuit in a directory that is accessible by a.OPTION
SEARCH=‘<lib_path>’ statement.
Create subcircuit libraries in a hierarchy. Typically, the top-level subcircuit fully
describes the input/output buffer; any hierarchy is buried inside. The buried
hierarchy can include model statements, lower-level components, and
parameter assignments. Your library cannot use .LIB or .INCLUDE
statements anywhere in the hierarchy.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
63
Chapter 3: Input Netlist and Data Entry
Subcircuit Call Statement Discrete Device Libraries
64
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
4
Elements
4
Describes the syntax for the basic elements of a circuit netlist in HSPICE or
HSPICE RF.
Elements are local and sometimes customized instances of a device model
specified in your design netlist.
For descriptions of the standard device models on which elements (instances)
are based, see the HSPICE Elements and Device Models Manual and
theHSPICE MOSFET Models Manual.
Passive Elements
This section describes the passive elements: resistors, capacitors, and
inductors.
Values for Elements
HSPICE RF accepts equation-based resistors and capacitors. You can specify
the value of a resistor or capacitor as an arbitrary equation, involving node
voltages or variable parameters. Unlike HSPICE, you cannot use parameters to
indirectly reference node voltages in HSPICE RF.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
65
Chapter 4: Elements
Passive Elements
Resistor Elements in a HSPICE or HSPICE RF Netlist
Rxxx n1 n2 <mname> Rval <TC1 <TC2><TC>> <SCALE=val> <M=val>
+ <AC=val> <DTEMP=val> <L=val> <W=val> <C=val>
+ <NOISE=val>
Rxxx n1 n2 <mname> <R=>resistance <<TC1=>val>
+ <<TC2=>val> <<TC=>val> <SCALE=val> <M=val>
+ <AC=val> <DTEMP=val> <L=val> <W=val>
+ <C=val> <NOISE=val>
Rxxx n1 n2 R=‘equation’ ...
Parameter
Description
Rxxx
Resistor element name. Must begin with R, followed by up to 1023
alphanumeric characters.
n1
Positive terminal node name.
n2
Negative terminal node name.
mname
Resistor model name. Use this name in elements, to reference a
resistor model.
TC
TC1 alias. The current definition overrides the previous definition.
TC1
First-order temperature coefficient for the resistor. See the “Passive
Device Models” chapter in the HSPICE Elements and Device Models
Manual for temperature-dependent relations.
TC2
Second-order temperature coefficient for the resistor.
SCALE
Element scale factor; scales resistance and capacitance by its value.
Default=1.0.
R=
resistance
Resistance value at room temperature. This can be:
■
■
■
■
■
66
a numeric value in ohms
a parameter in ohms
a function of any node voltages
a function of branch currents
any independent variables such as time, hertz, and temper
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Parameter
Description
M
Multiplier to simulate parallel resistors. For example, for two parallel
instances of a resistor, set M=2, to multiply the number of resistors by
2. Default=1.0.
AC
Resistance for AC analysis. Default=Reff.
DTEMP
Temperature difference between the element and the circuit, in degrees
Celsius. Default=0.0.
L
Resistor length in meters. Default=0.0, if you did not specify L in a
resistor model.
W
Resistor width. Default=0.0, if you did not specify W in the model.
C
Capacitance connected from node n2 to bulk. Default=0.0, if you did
not specify C in a resistor model.
user-defined Can be a function of any node voltages, element currents, temperature,
equation
frequency, or time
NOISE
■
■
NOISE=0, do not evaluate resistor noise.
NOISE=1, evaluate resistor noise (default).
Resistance can be a value (in units of ohms) or an equation. Required
parameters are the two nodes, and the resistance or model name. If you
specify other parameters, the node and model name must precede those
parameters. Other parameters can follow in any order. If you specify a resistor
model (see the “Passive Device Models” chapter in the HSPICE Elements and
Device Models Manual), the resistance value is optional.
HSPICE Examples
In the following example, the R1 resistor connects from the Rnode1 node to the
Rnode2 node, with a resistance of 100 ohms.
R1 Rnode1 Rnode2 100
The RC1 resistor connects from node 12 to node 17, with a resistance of 1
kilohm, and temperature coefficients of 0.001 and 0.
RC1 12 17 R=1k TC1=0.001 TC2=0
The Rterm resistor connects from the input node to ground, with a resistance
determined by the square root of the analysis frequency (non-zero for AC
analysis only).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
67
Chapter 4: Elements
Passive Elements
Rterm input gnd R=’sqrt(HERTZ)’
The Rxxx resistor, from node 98999999 to node 87654321, with a resistance of
1 ohm for DC and time-domain analyses, and 10 gigohms for AC analyses.
Rxxx 98999999 87654321 1 AC=1e10
HSPICE RF Examples
Some basic examples for HSPICE RF include:
■
R1 is a resistor whose resistance follows the voltage at node c.
R1 1 0 ‘v(c)’
■
R2 is a resistor whose resistance is the sum of the absolute values of nodes
c and d.
R2 1 0 ‘abs(v(c)) + abs(v(d))’
■
R3 is a resistor whose resistance is the sum of the rconst parameter, and
100 times tx1 for a total of 1100 ohms.
.PARAM rconst=100 tx1=10
R3 4 5 ‘rconst + tx1 * 100’
Linear Resistors
Rxxx node1 node2 < modelname > < R = > value < TC1=val >
+ < TC2=val > < W=val > < L=val > < M=val >
+ < C=val > < DTEMP=val > < SCALE=val >
68
Parameter
Description
Rxxx
Name of a resistor.
node1 and node2
Names or numbers of the connecting nodes.
modelname
Name of the resistor model.
value
Nominal resistance value, in ohms.
R
Resistance, in ohms, at room temperature.
TC1, TC2
Temperature coefficient.
W
Resistor width.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Parameter
Description
L
Resistor length.
M
Parallel multiplier.
C
Parasitic capacitance between node2 and the substrate.
DTEMP
Temperature difference between element and circuit.
SCALE
Scaling factor.
Example
R1 1 2 10.0
Rload 1 GND RVAL
.param rx=100
R3 2 3 RX TC1=0.001 TC2=0
RP X1.A X2.X5.B .5
.MODEL RVAL R
In the example above, R1 is a simple 10Ω linear resistor and Rload calls a
resistor model named RVAL, which is defined later in the netlist.
Note:
If a resistor calls a model, then you do not need to specify a constant
resistance, as you do with R1.
■
R3 takes its value from the RX parameter, and uses the TC1 and TC2
temperature coefficients, which become 0.001 and 0, respectively.
■
RP spans across different circuit hierarchies, and is 0.5Ω.
Behavioral Resistors in HSPICE or HSPICE RF
Rxxx n1 n2 . . . <R=> ‘equation’ . . .
Note:
The equation can be a function of any node voltage or branch current, and
any independent variables such as time, hertz, or temper.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
69
Chapter 4: Elements
Passive Elements
Example
R1 A B R=‘V(A) + I(VDD)’
Frequency-Dependent Resistors
Rxxx n1 n2 R=equation <CONVOLUTION=[0|1|2] <FBASE=value>
+ <FMAX=value>>
Parameter
CONVOLUTION
Description
Indicates which method is used.
■
■
■
FBASE
0 : Acts the same as the conventional method. This is the
default.
1 : Applies recursive convolution, and if the rational function
is not accurate enough, it switches to linear convolution.
2 : Applies linear convolution.
Specifies the lower bound of the transient analysis frequency.
For CONVOLUTION=1 mode, HSPICE starts sampling at this
frequency. For CONVOLUTION=2 mode, HSPICE uses this
value as the base frequency point for Inverse Fourier
Transformation.
For recursive convolution, the default value is 0Hz, and for
linear convolution, HSPICE uses the reciprocal of the transient
period.
FMAX
Specifies the possible maximum frequency of interest. The
default value is the frequency point where the function reaches
close enough to infinity value, assuming that the monotonous
function is approaching the infinity value and that it is taken at
10THz.
The equation should be a function of HERTZ. If
CONVOLUTION is turned on when a HERTZ keyword is not
used in the equation, it is automatically be turned off to let the
resistor behave as conventional.The equation can be a function
of temperature, but it cannot be node voltage or branch current
and time.
The equation can only be a function of time-independent variables such as
hertz, and temperature.
Example
R1 1 2 r='1.0 + 1e-5*sqrt(HERTZ)' CONVOLUTION=1
70
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Skin Effect Resistors
Rxxx n1 n2 R=value Rs=value
The Rs indicates the skin effect coefficient of the resistor.
The complex impedance of the resistor can be expressed as the following
equation:
R(f)=Ro + (1+j)*Rs*sqrt(f)
The Ro, j, and f are DC resistance, imaginably unit (j^2=-1) and frequency,
respectively.
Capacitors
Cxxx n1 n2 <mname> <C=>capacitance <<TC1=>val>
+ <<TC2=>val> <SCALE=val> <IC=val> <M=val>
+ <W=val> <L=val> <DTEMP=val>
Cxxx n1 n2 <C=>’equation’ <CTYPE=0|1>
+ <above_options...>
Polynomial form:
Cxxx n1 n2 POLY c0 c1... <above_options...>
Parameter
Description
Cxxx
Capacitor element name. Must begin with C, followed by up to 1023
alphanumeric characters.
n1
Positive terminal node name.
n2
Negative terminal node name.
mname
Capacitance model name. Elements use this name to reference a
capacitor.
C=capacitance
Capacitance at room temperature—a numeric value or a parameter
in farads.
TC1
First-order temperature coefficient for the capacitor. See the
“Passive Device Models” chapter in the HSPICE Elements and
Device Models Manual for temperature-dependent relations.
TC2
Second-order temperature coefficient for the capacitor.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
71
Chapter 4: Elements
Passive Elements
Parameter
Description
SCALE
Element scale parameter, scales capacitance by its value.
Default=1.0.
IC
Initial voltage across the capacitor, in volts. If you specify UIC in
the .TRAN statement, HSPICE or HSPICE RF uses this value as
the DC operating point voltage. The .IC statement overrides it.
M
Multiplier, used to simulate multiple parallel capacitors. Default=1.0
W
Capacitor width, in meters. Default=0.0, if you did not specify W in
a capacitor model.
L
Capacitor length, in meters. Default=0.0, if you did not specify L in
a capacitor model.
DTEMP
Element temperature difference from the circuit temperature, in
degrees Celsius. Default=0.0.
C=’equation’
Capacitance at room temperature, specified as a function of:
■
■
■
any node voltages
any branch currents
any independent variables such as time, hertz, and temper
CTYPE
Determines capacitance charge calculation for elements with
capacitance equations. If the C capacitance is a function of
V(n1<,n2>), set CTYPE=0. Use this setting correctly, to ensure
proper capacitance calculations, and correct simulation results.
Default=0.
POLY
Keyword, to specify capacitance as a non-linear polynomial.
c0 c1...
Coefficients of a polynomial, described as a function of the voltage
across the capacitor. c0 represents the magnitude of the 0th order
term, c1 represents the magnitude of the 1st order term, and so on.
You cannot use parameters as coefficient values.
You can specify capacitance as a numeric value, in units of farads, as an
equation, or as a polynomial of the voltage. The only required fields are the two
nodes, and the capacitance or model name.
72
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
■
If you use the parameter labels, the nodes and model name must precede
the labels. Other arguments can follow in any order.
■
If you specify a capacitor model (see the “Passive Device Models” chapter
in the HSPICE Elements and Device Models Manual), the capacitance
value is optional.
If you use an equation to specify capacitance, the CTYPE parameter
determines how HSPICE calculates the capacitance charge. The calculation is
different, depending on whether the equation uses a self-referential voltage
(that is, the voltage across the capacitor, whose capacitance is determined by
the equation).
To avoid syntax conflicts, if a capacitor model has the same name as a
capacitance parameter, HSPICE or HSPICE RF uses the model name.
Example 1
In the following example, C1 assumes its capacitance value from the model,
not the parameter.
.PARAMETER CAPXX=1
C1 1 2 CAPXX
.MODEL CAPXX C CAP=1
Example 2
In the following example, the C1 capacitors connect from node 1 to node 2, with
a capacitance of 20 picofarads:
C1 1 2 20p
In this next example, Cshunt refers to three capacitors in parallel, connected
from the node output to ground, each with a capacitance of 100 femtofarads.
Cshunt output gnd C=100f M=3
The Cload capacitor connects from the driver node to the output node. The
capacitance is determined by the voltage on the capcontrol node, times 1E-6.
The initial voltage across the capacitor is 0 volts.
Cload driver output C=’1u*v(capcontrol)’ CTYPE=1 IC=0v
The C99 capacitor connects from the in node to the out node. The capacitance
is determined by the polynomial C=c0 + c1*v + c2*v*v, where v is the voltage
across the capacitor.
C99 in out POLY 2.0 0.5 0.01
HSPICE® Simulation and Analysis User Guide
Y-2006.03
73
Chapter 4: Elements
Passive Elements
Linear Capacitors
Cxxx node1 node2 < modelname > < C=> value < TC1=val >
+ < TC2=val > <W=val > < L=val > < DTEMP=val >
+ < M=val > < SCALE=val > < IC=val >
Parameter
Description
Cxxx
Name of a capacitor. Must begin with C, followed by up to 1023
alphanumeric characters.
node1 and node2
Names or numbers of connecting nodes.
value
Nominal capacitance value, in Farads.
modelname
Name of the capacitor model.
C
Capacitance, in Farads, at room temperature.
TC1, TC2
Specifies the temperature coefficient.
W
Capacitor width.
L
Capacitor length.
M
Multiplier to simulate multiple parallel capacitors.
DTEMP
Temperature difference between element and circuit.
SCALE
Scaling factor.
IC
Initial capacitor voltage.
Example
Cbypass 1 0 10PF
C1 2 3 CBX
.MODEL CBX C
CB B 0 10P IC=4V
CP X1.XA.1 0 0.1P
In this example:
74
■
Cbypass is a straightforward, 10-picofarad (PF) capacitor.
■
C1, which calls the CBX model, does not have a constant capacitance.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
■
CB is a 10 PF capacitor, with an initial voltage of 4V across it.
■
CP is a 0.1 PF capacitor.
Frequency-Dependent Capacitors
You can specify frequency-dependent capacitors using the C=’equation’
with the HERTZ keyword. The HERTZ keyword represents the operating
frequency. In time domain analyses, an expression with the HERTZ keyword
behaves differently according to the value assigned to the CONVOLUTION
keyword.
Syntax
Cxxx n1 n2 C=’equation’ <CONVOLUTION=[0|1|2]
+ <FBASE=val> <FMAX=val>>
Parameter
Description
n1 n2
Names or numbers of connecting nodes.
equation
Expressed as a function of HERTZ. If CONVOLUTION=1 or 2
and HERTZ is not used in the equation, CONVOLUTION is
turned off and the capacitor behaves conventionally.
The equation can be a function of temperature, but it does not
support variables of node voltage, branch current, or time. If
these variables exist in the expression and CONVOLUTION=1 or
2, then only their values at the operating point are considered in
calculation.
CONVOLUTION
Specifies the method used.
■
■
0 (default): HERTZ=0 in time domain analysis.
1 or 2: performs Inverse Fast Fourier Transformation (IFFT)
linear convolution.
FBASE
Base frequency to use for transient analysis. This value becomes
the base frequency point for Inverse Fast Fourier Transformation
(IFFT) when CONVOLUTION=1 or 2. If you do not set this value,
the base frequency is a reciprocal value of the transient period.
FMAX
Maximum frequency to use for transient analysis. Used as the
maximum frequency point for Inverse Fourier Transformation. If
you do not set this value, the reciprocal value of RISETIME is
taken.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
75
Chapter 4: Elements
Passive Elements
Example
C1 1 2 C='1e-6 - HERTZ/1e16' CONVOLUTION=1 fbase=10
+ fmax=30meg
Behavioral Capacitors in HSPICE or HSPICE RF
Cxxx n1 n2 . . . C=‘equation’ CTYPE=0 or 1
Parameter
Description
CTYPE
Determines the calculation mode for elements that use capacitance
equations. Set this parameter carefully, to ensure correct simulation
results. HSPICE RF extends the definition and values of CTYPE,
relative to HSPICE:
■
■
■
CTYPE=0, if C depends only on its own terminal voltages—that is,
a function of V(n1<, n2>).
CTYPE=1, if C depends only on outside voltages or currents.
CTYPE=2, if C depends on both its own terminal and outside
voltages. This is the default for HSPICE RF. HSPICE does not
support C=2.
You can specify the capacitor value as a function of any node voltage or branch
current, and any independent variables such as time, hertz, and temper.
Example
C1 1 0 C=’1e-9*V(10)’ CTYPE=1
V10 10 0 PWL(0,1v t1,1v t2,4v)
DC Block Capacitors
Cxxx node1 node2 <C=> INFINITY
<IC=val>
When the capacitance of a capacitor is infinity, this element is called a “DC
block.” In HSPICE, you specify an INFINITY value for such capacitors.
HPSICE does not support any other capacitor parameters for DC block
elements, because HSPICE assumes that an infinite capacitor value is
independent of any scaling factors.
The DC block acts as an open circuit for all DC analyses. HSPICE calculates
the DC voltage across the nodes of the circuit. In all other (non-DC) analyses, a
DC voltage source of this value represents the DC block—HSPICE does not
allow dv/dt variations.
76
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Charge-Conserved Capacitors
Cxxx node1 node2 q=’expression’
HSPICE supports AC, DC, TRAN, and PZ analyses for charge-conserved
capacitors.
The expression supports the following parameters and variables:
■
■
Parameters
•
node voltages
•
branch currents
Variables
•
time
•
temper
•
hertz
Note:
The hertz variable is not supported in transient analyses.
Parameters must be used directly in an equation. HSPICE does not support
parameters that represent an equation containing variables.
Error Handling If you use an unsupported parameter in an expression,
HSPICE issues an error message and aborts the simulation. HSPICE ignores
unsupported analysis types and then issues warning a message.
Limitations
capacitors:
The following syntax does not support charge-conserving
Cxx node1 node2 C=’expression’
Capacitor equations are not implicitly converted to charge equations.
Example 1: Capacitance-based Capacitor
C1 a b C=‘Co*(1+alpha*V(a,b)’ ctype=0
You can obtain Q by integrating ‘C’ w.r.t V(a,b)
Example 2: Charge-based Capacitor
C1 a b Q=‘Co*V(a,b)(1+0.5*alpha*V(a,b))
HSPICE® Simulation and Analysis User Guide
Y-2006.03
77
Chapter 4: Elements
Passive Elements
Example 3: Capacitance-based Capactor
.option list node post
r1 1 2 100
r2 3 0 200
Vin 1 0 pulse(0 5v 1ns 2ns 2ns 10ns 20ns)
C1 2 3 c='cos(v(2,3)) + v(1,2)’ ctype=2
.tran 1ns 100ns
.print tran i(c1)
.end
Example 4: Charge-based Capacitor
.option list node post
r1 1 2 100
r2 3 0 200
Vin 1 0 pulse(0 5v 1ns 2ns 2ns 10ns 20ns)
C1 2 3 q='sin(v(2,3)) + v(2,3)*v(1,2)'
.tran 1ns 100ns
.print tran i(c1)
.end
Inductors
General form:
Lxxx n1 n2 <L=>inductance <mname> <<TC1=>val>
+ <<TC2=>val> <SCALE=val> <IC=val> <M=val>
+ <DTEMP=val> <R=val>
Lxxx n1 n2 L=‘equation’ <LTYPE=val> <above_options...>
Polynomial form:
Lxxx n1 n2 POLY c0 c1... <above_options...>
Magnetic winding form:
Lxxx n1 n2 NT=turns <above_options...>
78
Parameter
Description
Lxxx
Inductor element name. Must begin with L, followed by up to
1023 alphanumeric characters.
n1
Positive terminal node name.
n2
Negative terminal node name.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Parameter
Description
TC1
First-order temperature coefficient for the inductor. See the
“Passive Device Models” chapter in the HSPICE Elements and
Device Models Manual for temperature-dependent relations.
TC2
Second-order temperature coefficient for the inductor.
SCALE
Element scale parameter; scales inductance by its value.
Default=1.0.
IC
Initial current through the inductor, in amperes. HSPICE or
HSPICE RF uses this value as the DC operating point voltage,
when you specify UIC in the .TRAN statement. The .IC
statement overrides it.
L=inductance
Inductance value. This can be:
■
■
■
■
■
a numeric value, in henries
a parameter in henries
a function of any node voltages
a function of branch currents
any independent variables such as time, hertz, and
temper
M
Multiplier, used to simulate parallel inductors. Default=1.0.
DTEMP
Temperature difference between the element and the circuit, in
degrees Celsius. Default=0.0.
R
Resistance of the inductor, in ohms. Default=0.0.
L=‘equation’
Inductance at room temperature, specified as:
■
■
■
LTYPE
a function of any node voltages
a function of branch currents
any independent variables such as time, hertz, and
temper
Calculates inductance flux for elements, using inductance
equations. If the L inductance is a function of I(Lxxx), then set
LTYPE=0. Otherwise, set LTYPE=1. Use this setting correctly, to
ensure proper inductance calculations, and correct simulation
results. Default=0.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
79
Chapter 4: Elements
Passive Elements
Parameter
Description
POLY
Keyword that specifies the inductance, calculated by a
polynomial.
c0 c1...
Coefficients of a polynomial in the current, describing the
inductor value. c0 is the magnitude of the 0th order term, c1 is
the magnitude of the 1st order term, and so on.
NT=turns
Number of turns of an inductive magnetic winding.
mname
Saturable core model name. See the “Passive Device Models”
chapter in the HSPICE Elements and Device Models Manual for
model information.
In this syntax, the inductance can be either a value (in units of henries), an
equation, a polynomial of the current, or a magnetic winding. Required fields
are the two nodes, and the inductance or model name.
■
If you specify parameters, the nodes and model name must be first. Other
parameters can be in any order.
■
If you specify an inductor model (see the “Passive Device Models” chapter
in the HSPICE Elements and Device Models Manual), the inductance value
is optional.
Example 1
In the following example, the L1 inductor connects from the coilin node to the
coilout node, with an inductance of 100 nanohenries.
L1 coilin coilout 100n
Example 2
The Lloop inductor connects from node 12 to node 17. Its inductance is 1
microhenry, and its temperature coefficients are 0.001 and 0.
Lloop 12 17 L=1u TC1=0.001 TC2=0
Example 3
The Lcoil inductor connects from the input node to ground. Its inductance is
determined by the product of the current through the inductor, and 1E-6.
Lcoil input gnd L=’1u*i(input)’ LTYPE=0
80
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Example 4
The L99 inductor connects from the in node to the out node. Its inductance is
determined by the polynomial L=c0 + c1*i + c2*i*i, where i is the current
through the inductor. The inductor also has a specified DC resistance of 10
ohms.
L99 in out POLY 4.0 0.35 0.01 R=10
Example 5
The L inductor connects from node 1 to node, as a magnetic winding element,
with 10 turns of wire.
L 1 2 NT=10
Mutual Inductors
General form:
Kxxx Lyyy Lzzz <K=coupling | coupling>
Mutual core form:
Kaaa Lbbb <Lccc ... <Lddd>> mname <MAG=magnetization>
Parameter
Description
Kxxx
Mutual inductor element name. Must begin with K, followed by up
to 1023 alphanumeric characters.
Lyyy
Name of the first of two coupled inductors.
Lzzz
Name of the second of two coupled inductors.
K=coupling
Coefficient of mutual coupling. K is a unitless number, with
magnitude > 0 and < 1. If K is negative, the direction of coupling
reverses. This is equivalent to reversing the polarity of either of
the coupled inductors. Use the K=coupling syntax when using a
parameter value or an equation, and the keyword “k=” can be
omitted.
Kaaa
Saturable core element name. Must begin with K, followed by up
to 1023 alphanumeric characters.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
81
Chapter 4: Elements
Passive Elements
Parameter
Description
Lbbb, Lccc, Lddd
Names of the windings about the Kaaa core. One winding
element is required, and each winding element must use the
magnetic winding syntax. All winding elements with the same
magnetic core model should be written in one mutual inductor
statement in the netlist.
mname
Saturable core model name. (See the “Passive Device Models”
chapter in the HSPICE Elements and Device Models Manual for
more information.)
MAG=
Initial magnetization of the saturable core. You can set this to +1,
0, or -1, where +/- 1 refer to positive and negative values of the
BS model parameter. (See the “Passive Device Models” chapter
in the HSPICE Elements and Device Models Manual for more
information.)
magnetization
In this syntax, coupling is a unitless value, from zero to one, representing the
coupling strength. If you use parameter labels, the nodes and model name
must be first. Other arguments can be in any order. If you specify an inductor
model (see the “Passive Device Models” chapter in the HSPICE Elements and
Device Models Manual), the inductance value is optional.
You can determine the coupling coefficient, based on geometric and spatial
information. To determine the final coupling inductance, HSPICE or HSPICE
RF divides the coupling coefficient by the square-root of the product of the selfinductances.
When using the mutual inductor element to calculate the coupling between
more than two inductors, HSPICE or HSPICE RF can automatically calculate
an approximate second-order coupling. See the third example below for a
specific situation.
Note:
The automatic inductance calculation is an estimation, and is accurate for a
subset of geometries. The second-order coupling coefficient is the product
of the two first-order coefficients, which is not correct for many geometries.
Example 1
The Lin and Lout inductors are coupled, with a coefficient of 0.9.
K1 Lin Lout 0.9
82
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Example 2
The Lhigh and Llow inductors are coupled, with a coefficient equal to the value
of the COUPLE parameter.
Kxfmr Lhigh Llow K=COUPLE
■
The K1 mutual inductor couples L1 and L2.
■
The K2 mutual inductor couples L2 and L3.
Example 3
The coupling coefficients are 0.98 and 0.87. HSPICE or HSPICE RF
automatically calculates the mutual inductance between L1 and L3, with a
coefficient of 0.98*0.87=0.853.
K1 L1 L2 0.98
K2 L2 L3 0.87
Ideal Transformer
Kxxx Li Lj <k=IDEAL | IDEAL>
Ideal transformers use the IDEAL keyword with the K element to designate
ideal K transformer coupling.
This keyword activates the following equation set for non-DC values, which is
presented here with multiple coupled inductors. Ij is the current into the first
terminal of Lj.
V1/sqrt(L1)=V2/sqrt(L2)=V3/sqrt(L3)=V4/sqrt(L4)=...
(I1*sqrt(L1) + (I2*sqrt(L2) + (I3*sqrt(L3) + (I4*sqrt(L4) +
...=0
HSPICE can solve any I or V in terms of L ratios. DC is treated as expected—
inductors are treated as short circuits. Mutual coupling is ignored for DC.
Inductors that use the INFINITY keyword can be coupled with IDEAL K
elements. In this situation, all inductors involved must have the INFINITY
value, and for K=IDEAL, the ratio of all L values is unity. Then, for two L values:
v2= v1
i2 + i1=0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
83
Chapter 4: Elements
Passive Elements
Example 1
This example is a standard 5-pin ideal balun transformer subcircuit. Two pins
are grounded for standard operation. With all K values being IDEAL, the
absolute L values are not crucial—only their ratios are important.
**
**
all K's ideal
**
**
o----in**
Lin=1
** 0 o------**
.subckt BALUN1 in
Lin
in
gnd
Lo1
out1 gnd
Lo2
gnd
out2
K12
Lin Lo1
K13
Lin Lo2
K23
Lo1 Lo2
.ends
-----o out1
Lo1=.25
-----o 0
Lo2=.25
-----o out2
out1 out2
L=1
L=0.25
L=0.25
IDEAL
IDEAL
IDEAL
Example 2
This example is a 2-pin ideal 4:1 step-up balun transformer subcircuit with
shared DC path (no DC isolation). Input and output have a common pin, and
both inductors have the same value. Note that Rload=4*Rin.
**
**
all K's ideal
**in o-------------------o out=in
**
L1=1
**
-----o 0
**
L2=1
**
-----o out2
**
** With all K's ideal, the actual L's values are
** not important -- only their ratio to each other.
.subckt BALUN2 in out2
L1
in
gnd
L=1
L2
gnd out2 L=1
K12
L1
L2
IDEAL
.ends
84
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Example 3
This example is a 3-pin ideal balun transformer with shared DC path (no DC
isolation). All inductors have the same value (here set to unity).
**
**
all K's ideal -----o out1
**
Lo2=1
**
-----o 0
**
Lo1=1
**
-----o out2
**
in
Lin=1
**
o-------------------o in
**
.subckt BALUN3 in out1 out2
Lo2
gnd out1 L=1
Lo1
out2 gnd
L=1
Lin
in
out2 L=1
K12
Lin Lo1 IDEAL
K13
Lin Lo2 IDEAL
K23
Lo1 Lo2 IDEAL
.ends
Linear Inductors
Lxxx node1 node2 <L => inductance <TC1=val> <TC2=val>
+ <M=val> <DTEMP=val> <IC=val>
Parameter
Description
Lxxx
Name of an inductor.
node1 and node2
Names or numbers of the connecting nodes.
inductance
Nominal inductance value, in Henries.
L
Inductance, in Henries, at room temperature.
TC1, TC2
Temperature coefficient.
M
Multiplier for parallel inductors.
DTEMP
Temperature difference between the element and the circuit.
IC
Initial inductor current.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
85
Chapter 4: Elements
Passive Elements
Example:
LX A B 1E-9
LR 1 0 1u IC=10mA
■
LX is a 1 nH inductor.
■
LR is a 1 uH inductor, with an initial current of 10 mA.
Frequency-Dependent Inductors
You can specify frequency-dependent inductors using the L=’equation’ with
the HERTZ keyword. The HERTZ keyword represents the operating frequency.
In time domain analyses, an expression with the HERTZ keyword behaves
differently according to the value assigned to the CONVOLUTION keyword.
Syntax
Lxxx n1 n2 L=’equation’ <CONVOLUTION=[0|1|2] <FBASE=value>
+ <FMAX=value>>
Parameter
Description
Lxxx
Inductor element name. Must begin with L, followed by up to
1023 alphanumeric characters
n1 n2
Positive and negative terminal node names.
equation
The equation should be a function of HERTZ. If
CONVOLUTION is turned on when a HERTZ keyword is not
used in the equation, CONVOLUTION is automatically be
turned off and the inductor behaves conventionally.The
equation can be a function of temperature, but it does not
support variables of node voltage, branch current, or time. If
these variables exist in the equation with CONVOLUTION
turned on, only their values at the operating point are
considered in the calculation.
CONVOLUTION
Indicates which method is used.
■
■
■
86
0 (default): Acts the same as the conventional method.
1 : Applies recursive convolution, and if the rational function
is not accurate enough, it switches to linear convolution.
2 : Applies linear convolution.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Parameter
Description
FBASE
Specifies the lower bound of the transient analysis frequency.
■
■
■
■
FMAX
For CONVOLUTION=1 mode, HSPICE starts sampling at
this frequency.
For CONVOLUTION=2 mode, HSPICE uses this value as
the base frequency point for Inverse Fourier Transformation.
For recursive convolution, the default value is 0Hz.
For linear convolution, HSPICE uses the reciprocal of the
transient period.
Specifies the possible maximum frequency of interest. The
default value is the frequency point where the function reaches
close enough to infinity value, assuming that the monotonous
function is approaching the infinity value and that it is taken at
10THz.
Example
L1 1 2 L='0.5n + 0.5n/(1 + HERTZ/1e8)' CONVOLUTION=1 fbase=10
+ fmax=30meg
AC Choke Inductors
Syntax
Lxxx node1 node2
<L=> INFINITY
<IC=val>
When the inductance of an inductor is infinity, this element is called an “AC
choke.” In HSPICE, you specify an INFINITY value for inductors.
HSPICE does not support any other inductor parameters, because it assumes
that the infinite inductance value is independent of temperature and scaling
factors. The AC choke acts as a short circuit for all DC analyses and HSPICE
calculates the DC current through the inductor. In all other (non-DC) analyses,
a DC current source of this value represents the choke—HSPICE does not
allow di/dt variations.
To properly simulate power-line inductors with HSPICE RF, either set them to
analog mode or invoke the SIM_RAIL option:
.OPTION SIM_ANALOG=“L1”
-or.OPTION SIM_RAIL=ON
HSPICE® Simulation and Analysis User Guide
Y-2006.03
87
Chapter 4: Elements
Passive Elements
Reluctors
Syntax
Reluctance Inline Form
Lxxx n1p n1n ... nNp nNn
+ RELUCTANCE=(r1, c1, val1, r2, c2, val2, ... , rm, cm, valm)
+ <SHORTALL=yes | no> <IGNORE_COUPLING=yes | no>
Reluctance External File Form
Lxxx n1p n1n ... nNp nNn RELUCTANCE
+ FILE="<filename1>" [FILE="<filename2>" [...]]
+ <SHORTALL=yes | no> <IGNORE_COUPLING=yes | no>
88
Parameter
Description
Lxxx
Name of a reluctor. Must begin with L, followed by up to 1023
alphanumeric characters
n1p n1n ...
nNp nNn
Names of the connecting terminal nodes. The number of
terminals must be even. Each pair of ports represnets the
location of an inductor.
RELUCTANCE
Keyword to specify reluctance (inverse inductance).
r1, c1, val1,
r2, c2, val2, ...
rm, cm, valm
Reluctance matrix data. In general, K will be sparse and only
non-zero values in the matrix need be given. Each matrix entry
is represented by a triplet (r,c,val). The value r and c are
integers referring to a pair of inductors from the list of terminal
nodes. If there are 2*N terminal nodes, there will be N
inductors, and the r and c values must be in the range [1,N].
The val value is a reluctance value for the (r,c) matrix location,
and the unit for reluctance is the inverse Henry (H-1).
Only terms along and above the diagonal are specified for the
reluctance_matrix.
The simulator fills in the lower triangle to ensure symmetry. If
you specify lower diagonal terms, the simulator converts that
entry to the appropriate upper diagonal term.
If multiple entries are supplied for the same (r,c) location, then
only the first one is used, and a warning will be issued
indicating that some entries are ignored.
All diagonal entries of the reluctance matrix must be assigned
a positive value.
The reluctance matrix should be positive definite.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Passive Elements
Parameter
Description
FILE="<filename1>"
For the external file format, the data files should contain three
columns of data. Each row should contain an (r,c,val) triplet
separated by white space. The r, c, and val values may be
expressions surrounded by single quotes. Multiple files may be
specified to allow the reluctance data to be spread over several
files if necessary.
SHORTALL
■
■
IGNORE_COUPLIN
G
■
■
SHORTALL=yes, all inductors in this model are converted
to short circuits, and all reluctance matrix values are
ignored.
SHORTALL=no (default), inductors are not converted to
short circuits, and reluctance matrix values are not ignored.
IGNORE_COUPLING=yes, all off-diagonal terms are
ignored (that is, set to zero).
IGNORE_COUPLING=no (default), off-diagonal terms are
not ignored.
Example
This example has 9 segments (or ports) with 12 nodes, and can potentially
generate a 9x9 reluctance matrix with 81 elements.
L_ThreeNets a 1 1 2 2 a_1 b 4 4 5 5 b_1 c 7 7 8 8 c_1
+ RELUCTANCE=(
+ 1 1
103e9
+ 1 4
-34.7e9
+ 1 7
-9.95e9
+ 4 4
114e9
+ 4 7
-34.7e9
+ 7 7
103e9
+ 2 2
103e9
+ 2 5
-34.7e9
+ 2 8
-9.95e9
+ 5 5
114e9
+ 5 8
-34.7e9
+ 8 8
103e9
+ 3 3
103e9
+ 3 6
-34.7e9
+ 3 9
-9.95e9
+ 6 6
114e9
+ 6 9
-34.7e9
+ 9 9
103e9 )
+ SHORTALL = no IGNORE_COUPLING = no
HSPICE® Simulation and Analysis User Guide
Y-2006.03
89
Chapter 4: Elements
Passive Elements
Alternatively, the same element could be specified by using:
L_ThreeNets a 1 1 2 2 a_1 b 4 4 5 5 b_1 c 7 7 8 8 c_1 RELUCTANCE
+ FILE="reluctance.dat" SHORTALL = no IGNORE_COUPLING = no
Where reluctance.dat contains:
+
+
+
+
+
+
+
+
+
+
+
+
+
+
+
+
+
+
1
1
1
4
4
7
2
2
2
5
5
8
3
3
3
6
6
9
1
4
7
4
7
7
2
5
8
5
8
8
3
6
9
6
9
9
103e9
-34.7e9
-9.95e9
114e9
-34.7e9
103e9
103e9
-34.7e9
-9.95e9
114e9
-34.7e9
103e9
103e9
-34.7e9
-9.95e9
114e9
-34.7e9
103e9
The following shows the mapping between the port numbers and node pairs:
------------------------------------------------------------------------------------|Ports
|
1
|
2
|
3
|
4
|
5
|
6
|
7
|
8
|
9
|
|Node pairs | (a,1) | (1,2) |(2,a_1)| (b,4) | (4,5) |(5,b_1)| (c,7) | (7,8) |(8,c_1)|
-------------------------------------------------------------------------------------
90
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Active Elements
Active Elements
This section describes the passive elements: diodes and transistors.
Diode Element
Geometric (LEVEL=1) or Non-Geometric (LEVEL=3) form:
Dxxx nplus nminus mname <<AREA=>area> <<PJ=>val>
+ <WP=val> <LP=val> <WM=val> <LM=val> <OFF>
+ <IC=vd> <M=val> <DTEMP=val>
Dxxx nplus nminus mname <W=width> <L=length> <WP=val>
+ <LP=val> <WM=val> <LM=val> <OFF> <IC=vd> <M=val>
+ <DTEMP=val>
Fowler-Nordheim (LEVEL=2) form:
Dxxx nplus nminus mname <W=val <L=val>> <WP=val>
+ <OFF> <IC=vd> <M=val>
Parameter
Description
Dxxx
Diode element name. Must begin with D, followed by up to 1023
alphanumeric characters.
nplus
Positive terminal (anode) node name. The series resistor for the
equivalent circuit is attached to this terminal.
nminus
Negative terminal (cathode) node name.
mname
Diode model name reference.
AREA
Area of the diode (unitless for LEVEL=1 diode, and square meters for
LEVEL=3 diode). This affects saturation currents, capacitances, and
resistances (diode model parameters are IK, IKR, JS, CJO, and RS).
The SCALE option does not affect the area factor for the LEVEL=1
diode. Default=1.0. Overrides AREA from the diode model. If you do not
specify the AREA, HSPICE or HSPICE RF calculates it from the width
and length.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
91
Chapter 4: Elements
Active Elements
Parameter
Description
PJ
Periphery of junction (unitless for LEVEL=1 diode, and meters for
LEVEL=3 diode). Overrides PJ from the diode model. If you do not
specify PJ, HSPICE or HSPICE RF calculates it from the width and
length specifications.
WP
Width of polysilicon capacitor, in meters (for LEVEL=3 diode only).
Overrides WP in the diode model. Default=0.0.
LP
Length of polysilicon capacitor, in meters (for LEVEL=3 diode only).
Overrides LP in the diode model. Default=0.0.
WM
Width of metal capacitor, in meters (for LEVEL=3 diode only). Overrides
WM in the diode model. Default=0.0.
LM
Length of metal capacitor, in meters (for LEVEL=3 diode only).
Overrides LM in the diode model. Default=0.0.
OFF
Sets the initial condition for this element to OFF, in DC analysis.
Default=ON.
IC=vd
Initial voltage, across the diode element. Use this value when you
specify the UIC option in the .TRAN statement. The .IC statement
overrides this value.
M
Multiplier, to simulate multiple diodes in parallel. The M setting affects
all currents, capacitances, and resistances. Default=1.
DTEMP
The difference between the element temperature and the circuit
temperature, in degrees Celsius. Default=0.0.
W
Width of the diode, in meters (LEVEL=3 diode model only)
L
Length of the diode, in meters (LEVEL=3 diode model only)
You must specify two nodes and a model name. If you specify other
parameters, the nodes and model name must be first and the other parameters
can appear in any order.
Example 1
The D1 diode, with anode and cathode, connects to nodes 1 and 2. Diode1
specifies the diode model.
D1 1 2 diode1
92
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Active Elements
Example 2
The Dprot diode, with anode and cathode, connects to both the output node
and ground, references the firstd diode model, and specifies an area of 10
(unitless for LEVEL=1 model). The initial condition has the diode OFF.
Dprot output gnd firstd 10 OFF
Example 3
The Ddrive diode, with anode and cathode, connects to the driver and output
nodes. The width and length are 500 microns. This diode references the
model_d diode model.
Ddrive driver output model_d W=5e-4 L=5e-4 IC=0.2
Bipolar Junction Transistor (BJT) Element
Qxxx nc nb ne <ns> mname <area> <OFF>
+ <IC=vbeval,vceval> <M=val> <DTEMP=val>
Qxxx nc nb ne <ns> mname <AREA=area> <AREAB=val>
+ <AREAC=val> <OFF> <VBE=vbeval> <VCE=vceval>
+ <M=val> <DTEMP=val>
Parameter
Description
Qxxx
BJT element name. Must begin with Q, then up to 1023 alphanumeric
characters.
nc
Collector terminal node name.
nb
Base terminal node name.
ne
Emitter terminal node name.
ns
Substrate terminal node name, which is optional. You can also use the
BULK parameter to set this name in the BJT model.
mname
BJT model name reference.
area,
AREA=area
Emitter area multiplying factor, which affects currents, resistances, and
capacitances. Default=1.0.
OFF
Sets initial condition for this element to OFF, in DC analysis.
Default=ON.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
93
Chapter 4: Elements
Active Elements
Parameter
Description
IC=vbeval,
Initial internal base-emitter voltage (vbeval) and collector-emitter
vceval, VBE, voltage (vceval). HSPICE or HSPICE RF uses this value when
VCE
the .TRAN statement includes UIC. The .IC statement overrides it.
M
Multiplier, to simulate multiple BJTs in parallel. The M setting affects all
currents, capacitances, and resistances. Default=1.
DTEMP
The difference between the element temperature and the circuit
temperature, in degrees Celsius. Default=0.0.
AREAB
Base area multiplying factor, which affects currents, resistances, and
capacitances. Default=AREA.
AREAC
Collector area multiplying factor, which affects currents, resistances,
and capacitances. Default=AREA.
The only required fields are the collector, base, and emitter nodes, and the
model name. The nodes and model name must precede other fields in the
netlist.
Example 1
In the Q1 BJT element below:
Q1 1 2 3 model_1
■
The collector connects to node 1.
■
The base connects to node 2.
■
The emitter connects to node 3.
■
model_1 references the BJT model.
Example 2
In the following Qopamp1 BJT element:
Qopamp1 c1 b3 e2 s 1stagepnp AREA=1.5 AREAB=2.5
AREAC=3.0
94
■
The collector connects to the c1 node.
■
The base connects to the b3 node.
■
The emitter connects to the e2 node.
■
The substrate connects to the s node.
■
1stagepnp references the BJT model.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Active Elements
■
The AREA area factor is 1.5.
■
The AREAB area factor is 2.5.
■
The AREAC area factor is 3.0.
Example 3
In the Qdrive BJT element below:
Qdrive driver in output model_npn 0.1
■
The collector connects to the driver node.
■
The base connects to the in node.
■
The emitter connects to the output node.
■
model_npn references the BJT model.
■
The area factor is 0.1.
JFETs and MESFETs
Jxxx nd ng ns <nb> mname <<<AREA>=area | <W=val>
+ <L=val>> <OFF> <IC=vdsval,vgsval> <M=val>
+ <DTEMP=val>
Jxxx nd ng ns <nb> mname <<<AREA>=area> | <W=val>
+ <L=val>> <OFF> <VDS=vdsval> <VGS=vgsval>
+ <M=val> <DTEMP=val>
Parameter
Description
Jxxx
JFET or MESFET element name. Must begin with J, followed by up
to 1023 alphanumeric characters.
nd
Drain terminal node name
ng
Gate terminal node name
ns
Source terminal node name
nb
Bulk terminal node name, which is optional.
mname
JFET or MESFET model name reference
HSPICE® Simulation and Analysis User Guide
Y-2006.03
95
Chapter 4: Elements
Active Elements
Parameter
Description
area,
AREA=area
Area multiplying factor that affects the BETA, RD, RS, IS, CGS, and
CGD model parameters. Default=1.0, in units of square meters.
W
FET gate width in meters
L
FET gate length in meters
OFF
Sets initial condition to OFF for this element, in DC analysis.
Default=ON.
IC=vdsval,
vgsval, VDS,
VGS
Initial internal drain-source voltage (vdsval) and gate-source voltage
(vgsval). Use this argument when the .TRAN statement contains
UIC. The .IC statement overrides it.
M
Multiplier to simulate multiple JFETs or MESFETs in parallel. The M
setting affects all currents, capacitances, and resistances.
Default=1.
DTEMP
The difference between the element temperature and the circuit
temperature, in degrees Celsius. Default=0.0.
Only drain, gate, and source nodes, and model name fields are required. Node
and model names must precede other fields.
Example 1
In the J1 JFET element below:
J1 1 2 3 model_1
■
The drain connects to node 1.
■
The source connects to node 2.
■
The gate connects to node 3.
■
model_1 references the JFET model.
Example 2
In the following Jopamp1 JFET element:
Jopamp1 d1 g3 s2 b 1stage AREA=100u
96
■
The drain connects to the d1 node.
■
The source connects to the g3 node.
■
The gate connects to the s2 node.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Active Elements
■
1stage references the JFET model.
■
The area is 100 microns.
Example 3
In the Jdrive JFET element below:
Jdrive driver in output model_jfet W=10u L=10u
■
The drain connects to the driver node.
■
The source connects to the in node.
■
The gate connects to the output node.
■
model_jfet references the JFET model.
■
The width is 10 microns.
■
The length is 10 microns.
MOSFETs
Mxxx nd ng ns <nb> mname <<L=>length> <<W=>width>
+ <AD=val> AS=val> <PD=val> <PS=val>
+ <NRD=val> <NRS=val> <RDC=val> <RSC=val> <OFF>
+ <IC=vds,vgs,vbs> <M=val> <DTEMP=val>
+ <GEO=val> <DELVTO=val>
.OPTION WL
Mxxx nd ng ns <nb> mname <width> <length> <other_options...>
Parameter
Description
Mxxx
MOSFET element name. Must begin with M, followed by up to 1023
alphanumeric characters.
nd
Drain terminal node name.
ng
Gate terminal node name.
ns
Source terminal node name.
nb
Bulk terminal node name, which is optional. To set this argument in the
MOSFET model, use the BULK parameter.
mname
MOSFET model name reference
HSPICE® Simulation and Analysis User Guide
Y-2006.03
97
Chapter 4: Elements
Active Elements
98
Parameter
Description
L
MOSFET channel length, in meters. This parameter overrides
.OPTION DEFL, with a maximum value of 0.1m. Default=DEFL.
W
MOSFET channel width, in meters. This parameter overrides .OPTION
DEFW. Default=DEFW.
AD
Drain diffusion area. Overrides .OPTION DEFAD. Default=DEFAD, if
you set the ACM=0 model parameter.
AS
Source diffusion area. Overrides .OPTION DEFAS. Default=DEFAS, if
you set the ACM=0 model parameter.
PD
Perimeter of drain junction, including channel edge. Overrides
.OPTION DEFPD. Default=DEFAD, if you set the ACM=0 or 1 model
parameter. Default=0.0, if you set ACM=2 or 3.
PS
Perimeter of source junction, including channel edge. Overrides
.OPTION DEFPS. Default=DEFAS, if you set the ACM=0 or 1 model
parameter. Default=0.0, if you set ACM=2 or 3.
NRD
Number of squares of drain diffusion for resistance calculations.
Overrides .OPTION DEFNRD. Default=DEFNRD, if you set ACM=0 or
1 model parameter. Default=0.0, if you set ACM=2 or 3.
NRS
Number of squares of source diffusion for resistance calculations.
Overrides .OPTION DEFNRS. Default=DEFNRS when you set the
MOSFET model parameter ACM=0 or 1. Default=0.0, when you set
ACM=2 or 3.
RDC
Additional drain resistance due to contact resistance, in units of ohms.
This value overrides the RDC setting in the MOSFET model
specification. Default=0.0.
RSC
Additional source resistance due to contact resistance, in units of
ohms. This value overrides the RSC setting in the MOSFET model
specification. Default=0.0.
OFF
Sets initial condition for this element to OFF, in DC analysis.
Default=ON. This command does not work for depletion devices.
IC=vds, vgs,
vbs
Initial voltage across external drain and source (vds), gate and source
(vgs), and bulk and source terminals (vbs). Use these arguments
with .TRAN UIC. .IC statements override these values.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Active Elements
Parameter
Description
M
Multiplier, to simulate multiple MOSFETs in parallel. Affects all channel
widths, diode leakages, capacitances, and resistances. Default=1.
DTEMP
The difference between the element temperature and the circuit
temperature, in degrees Celsius. Default=0.0.
GEO
Source/drain sharing selector for a MOSFET model parameter value of
ACM=3. Default=0.0.
DELVTO
Zero-bias threshold voltage shift. Default=0.0.
The only required fields are the drain, gate and source nodes, and the model
name. The nodes and model name must precede other fields in the netlist. If
you did not specify a label, use the second syntax with the .OPTION WL
statement, to exchange the width and length options.
Example
In the following M1 MOSFET element:
M1 1 2 3 model_1
■
The drain connects to node 1.
■
The gate connects to node 2.
■
The source connects to node 3.
■
model_1 references the MOSFET model.
In the following Mopamp1 MOSFET element:
Mopamp1 d1 g3 s2 b 1stage L=2u W=10u
■
The drain connects to the d1 node.
■
The gate connects to the g3 node.
■
The source connects to the s2 node.
■
1stage references the MOSFET model.
■
The length of the gate is 2 microns.
■
The width of the gate is 10 microns.
In the following Mdrive MOSFET element:
Mdrive driver in output bsim3v3 W=3u L=0.25u DTEMP=4.0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
99
Chapter 4: Elements
Transmission Lines
■
The drain connects to the driver node.
■
The gate connects to the in node.
■
The source connects to the output node.
■
bsim3v3 references the MOSFET model.
■
The length of the gate is 3 microns.
■
The width of the gate is 0.25 microns.
■
The device temperature is 4 degrees Celsius higher than the circuit
temperature.
Transmission Lines
A transmission line is a passive element that connects any two conductors, at
any distance apart. One conductor sends the input signal through the
transmission line, and the other conductor receives the output signal from the
transmission line. The signal that is transmitted from one end of the pair to the
other end, is voltage between the conductors.
Examples of transmission lines include:
■
Power transmission lines
■
Telephone lines
■
Waveguides
■
Traces on printed circuit boards and multi-chip modules (MCMs)
■
Bonding wires in semiconductor IC packages
■
On-chip interconnections
W Element
The W element supports five different formats to specify the transmission line
properties:
■
100
Model 1: RLGC-Model specification.
•
Internally specified in a .model statement.
•
Externally specified in a different file.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
■
Model 2: U-Model specification.
•
RLGC input for up to five coupled conductors.
•
Geometric input (planer, coax, twin-lead).
•
Measured-parameter input.
•
Skin effect.
■
Model 3: Built-in field solver model.
■
Model 4: Frequency-dependent tabular model.
■
Model 5: S Parameter Model
W Element Statement
The general syntax for a lossy (W Element) transmission line element is:
RLGC file form:
Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>>
+ refout <RLGCfile=filename> N=val L=val
U Model form:
Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>>
+ refout <Umodel=modelname> N=val L=val
Field solver form:
Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>>
+ refout <FSmodel=modelname> N=val L=val
The number of ports on a single transmission line are not limited. You must
provide one input and output port, the ground references, a model or file
reference, a number of conductors, and a length. HSPICE RF does not support
the Field Solver form of the W element.
S Model form:
Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>>
+ refout <Smodel=modelname> <NODEMAP=XiYj...> N=val L=val
HSPICE® Simulation and Analysis User Guide
Y-2006.03
101
Chapter 4: Elements
Transmission Lines
Table Model form:
Wxxx in1 in2 <...inx>> refin out1 <out2 <...outx>>
+ refout N=val L=val TABLEMODEL=name
Parameter
Description
Wxxx
Lossy (W Element) transmission line element name. Must start
with W, followed by up to 1023 alphanumeric characters.
inx
Signal input node for xth transmission line (in1 is required).
refin
Ground reference for input signal
outx
Signal output node for the xth transmission line (each input port
must have a corresponding output port).
refout
Ground reference for output signal.
N
Number of conductors (excluding the reference conductor).
L
Physical length of the transmission line, in units of meters.
RLGCfile=filename
File name reference for the file containing the RLGC
information for the transmission lines (for syntax, see “Using
the W Element” in the HSPICE Signal Integrity Guide).
Umodel=modelname U-model lossy transmission-line model reference name. A
lossy transmission line model, used to represent the
characteristics of the W-element transmission line.
FSmodel=
modelname
102
Internal field solver model name. References the PETL internal
field solver as the source of the transmission-line
characteristics (for syntax, see “Using the Field Solver
Model”chapter in the HSPICE Signal Integrity Guide).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Parameter
Description
NODEMAP
String that assigns each index of the S parameter matrix to one
of the W Element terminals. This string must be an array of
pairs that consists of a letter and a number, (for example, Xn),
where
■
X= I, i, N, or n to indicate near end (input side) terminal of
the W element
■
X= O, i, F, or f to indicate far end (output side) terminal of the
W element.
The default value for NODEMAP is "I1I2I3...InO1O2O3...On"
Smodel
S Model name reference, which contains the S parameters of
the transmission lines (for the S Model syntax, see the HSPICE
Signal Integrity Guide).
TABLEMODEL
Name of the frequency-dependent tabular model.
Example 1
The W1 lossy transmission line connects the in node to the out node:
W1 in gnd out gnd RLGCfile=cable.rlgc N=1 L=5
Where,
■
Both signal references are grounded
■
The RLGC file is named cable.rlgc
■
The transmission line is 5 meters long.
Example 2
The Wcable element is a two-conductor lossy transmission line:
Wcable in1 in2 gnd out1 out2 gnd Umodel=umod_1 N=2
+ L=10
Where,
■
in1 and in2 input nodes connect to the out1 and out2 output node
■
Both signal references are grounded.
■
umod_1 references the U-model.
■
The transmission line is 10 meters long.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
103
Chapter 4: Elements
Transmission Lines
Example 3
The Wnet1 element is a five-conductor lossy transmission line:
Wnet1 i1 i2 i3 i4 i5 gnd o1 gnd o3 gnd o5 gnd
+ FSmodel=board1 N=5 L=1m
Where,
■
The i1, i2, i3, i4 and i5 input nodes connect to the o1, o3, and o5 output
nodes.
■
The i5 input and three outputs (o1, o3, and o5) are all grounded.
■
board1 references the Field Solver model.
■
The transmission line is 1 millimeter long.
Example 4: S Model Example
Wnet1 i1 i2 gnd o1 o2 gnd
+ Smodel=smod_1 nodemap=i1i2o1o2
+ N=2 L=10m
Where,
■
in1 and in2 input nodes connect to the out1 and out2 output node.
■
Both signal references are grounded.
■
smod_1 references the S Model.
■
The transmission line is 10 meters long.
You can specify parameters in the W Element card in any order. You can
specify the number of signal conductors, N, after the node list. You can also mix
nodes and parameters in the W Element card.
You can specify only one of the RLGCfile, FSmodel, Umodel, or Smodel
models, in a single W Element card.
Figure 13 shows node numbering for the element syntax.
104
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Figure 13
Terminal Node Numbering for the W Element
N+1 conductor line
[i1]1
1.1 [i ]
12
1.2
[i1]N
1.N
1’
[v1]1
R(f), L(f), G(f), C(f)
[v2]1
[v1]2
Signal Conductors
[v2]2
.
.
.
.
.
.
[v1]N
+
_
Reference conductor
[i2]1
[i2]2
.
.
.
2.2
[i2]N
2.N
[v2]N
+
_
0
2.1
2’
x
For additional information about the W element, see the “Modeling Coupled
Transmission Lines Using the W Element” chapter in the HSPICE Signal
Integrity User Guide.
Lossless (T Element)
General form:
Txxx in refin out refout Z0=val TD=val <L=val>
+ <IC=v1,i1,v2,i2>
Txxx in refin out refout Z0=val F=val <NL=val>
+ <IC=v1,i1,v2,i2>
U Model form:
Txxx in refin out refout mname L=val
Parameter
Description
Txxx
Lossless transmission line element name. Must begin with T,
followed by up to 1023 alphanumeric characters.
in
Signal input node.
refin
Ground reference for the input signal.
out
Signal output node.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
105
Chapter 4: Elements
Transmission Lines
refout
Ground reference for the output signal.
Z0
Characteristic impedance of the transmission line.
TD
Signal delay from a transmission line, in seconds per meter.
L
Physical length of the transmission line, in units of meters.
Default=1.
IC=v1,i1,v2,i2
Initial conditions of the transmission line. Specify the voltage on
the input port (v1), current into the input port (i1), voltage on the
output port (v2), and the current into the output port (i2).
F
Frequency at which the transmission line has the electrical length
specified in NL.
NL
Normalized electrical length of the transmission line (at the
frequency specified in the F parameter), in units of wavelengths
per line length. Default=0.25, which is a quarter-wavelength.
mname
U-model reference name. A lossy transmission line model,
representing the characteristics of the lossless transmission line.
Only one input and output port is allowed.
Example 1
The T1 transmission line connects the in node to the out node:
T1 in gnd out gnd Z0=50 TD=5n L=5
■
Both signal references are grounded.
■
Impedance is 50 ohms.
■
The transmission delay is 5 nanoseconds per meter.
■
The transmission line is 5 meters long.
Example 2
The Tcable transmission line connects the in1 node to the out1 node:
Tcable in1 gnd out1 gnd Z0=100 F=100k NL=1
106
■
Both signal references are grounded.
■
Impedance is 100 ohms.
■
The normalized electrical length is 1 wavelength at 100 kHz.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Example 3
The Tnet1 transmission line connects the driver node to the output node:
Tnet1 driver gnd output gnd Umodel1 L=1m
■
Both signal references are grounded.
■
Umodel1 references the U-model.
■
The transmission line is 1 millimeter long.
Ideal Transmission Line
For the ideal transmission line, voltage and current will propagate without loss
along the length of the line (±x direction) with spatial and time-dependence
given according to the following equation:
v ( x, t ) = Re [ Ae
j ( ωt – βx )
+ Be
j ( ϖt + βx )
]
B j ( ωt + βx )
A j ( ωt – βx ) ----v ( x, t ) = Re ----- e
– e
Z0
Z0
The A represents the incident voltage, B represents the reflected voltage, Z0 is
the characteristic impeadance, and β is the propagation constant. The latter are
related to the transmission line inductance (L) and capacitance (C) by the
following equation:
Z0 =
L--C
β = ω LC
The L and C terms are in per-unit-length units (Henries/meter, Farads/meter).
The following equation gives the phase velocity:
ω
1
υ ρ = ---- = ----------β
LC
At the end of the transmission line ( x = l ), the propagation term βl becomes
the following equation:
l
βl = ω LC ⋅ l = ω ----vp
HSPICE® Simulation and Analysis User Guide
Y-2006.03
107
Chapter 4: Elements
Transmission Lines
This is equivalent to an ideal delay with the following value:
l- =
T = ----VP
LC ⋅ l
Where,
T : absolute time delay (sec)
l : physical length (L) (meters)
VP : phase velocity (meters/sec)
Using standard distance=velocity*time relationships, the HSPICE T element
parameter values are related to these terms according to:
1V P = f ⋅ λ = --td
Where,
f
: frequency
λ
: wavelength
td
: relative time delay (TD) (sec/meter)
l - = t ⋅ l = -------l - = l-------⁄λ =
T = ----d
Vp
f⋅λ
f
LC ⋅ l
Where,
l
: physical length (L) (meters)
l⁄λ
f
: normalized length (NL)
: frequency at NL (F) (Hz)
T = TD ⋅ L = NL
------- =
L
LC ⋅ L
HSPICE therefore allows you to specify a transmission line in three different
ways:
■
Z0, TD, L
■
Z0, NL, F
■
108
L- and LC values taken from a U model.
L, with --C
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Lossy (U Element)
Uxxx in1 <in2 <...in5>> refin out1 <out2 <...out5>>
+ refout mname L=val <LUMPS=val>
Parameter
Description
Uxxx
Lossy (U Element) transmission line element name. Must begin with U,
followed by up to 1023 alphanumeric characters.
inx
Signal input node for the xth transmission line (in1 is required).
refin
Ground reference for the input signal.
outx
Signal output node for the xth transmission line (each input port must
have a corresponding output port).
refout
Ground reference for the output signal.
mname
Model reference name for the U-model lossy transmission-line.
L
Physical length of the transmission line, in units of meters.
LUMPS
Number of lumped-parameter sections used to simulate the element.
In this syntax, the number of ports on a single transmission line is limited to five
in and five out. One input and output port, the ground references, a model
reference, and a length are all required.
Example 1
The U1 transmission line connects the in node to the out node:
U1 in gnd out gnd umodel_RG58 L=5
■
Both signal references are grounded.
■
umodel_RG58 references the U-model.
■
The transmission line is 5 meters long.
Example 2
The Ucable transmission line connects the in1 and in2 input nodes to the out1
and out2 output nodes:
Ucable in1 in2 gnd out1 out2 gnd twistpr L=10
HSPICE® Simulation and Analysis User Guide
Y-2006.03
109
Chapter 4: Elements
Transmission Lines
■
Both signal references are grounded.
■
twistpr references the U-model.
■
The transmission line is 10 meters long.
Example 3
The Unet1 element is a five-conductor lossy transmission line:
Unet1 i1 i2 i3 i4 i5 gnd o1 gnd o3 gnd o5 gnd Umodel1 L=1m
■
The i1, i2, i3, i4, and i5 input nodes connect to the o1, o3, and o5 output
nodes.
■
The i5 input, and the three outputs (o1, o3, and o5) are all grounded.
■
Umodel1 references the U-model.
■
The transmission line is 1 millimeter long.
Frequency-Dependent Multi-Terminal S Element
The S element uses the following parameters to define a frequency-dependent,
multi-terminal network:
■
S (scattering)
■
Y (admittance)
■
Z (impedance)
You can use an S element in the following types of analyses:
■
DC
■
AC
■
Transient
■
Small Signal
For a description of the S parameter and SP model analysis, see the
“S Parameter Modeling Using the S Element” chapter in the HSPICE Signal
Integrity Guide.
S Element Syntax (HSPICE):
Sxxx nd1 nd2 ... ndN ndRef
+ <MNAME=Smodel_name> <FQMODEL=sp_model_name>
+ <TYPE=[s|y]> <Zo=[value|vector_value]>
+ <FBASE=base_frequency> <FMAX=maximum_frequency>
+ <PRECFAC=val> <DELAYHANDLE=[1|0|ON|OFF]>
110
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
+
+
+
+
+
+
<DELAYFREQ=val>
<INTERPOLATION=STEP|LINEAR|SPLINE>
<INTDATTYP =[RI|MA|DBA]> <HIGHPASS=value>
<LOWPASS=value> <MIXEDMODE=[0|1]>
<DATATYPE=data_string>
<DTEMP=val> <NOISE=[1|0]>
S Element Syntax (HSPICE RF):
Sxxx nd1 nd2 ... ndN [ndR] s_model_name
S model Syntax (HSPICE):
.MODEL S_model_name S
+ N=dimension
+ [FQMODEL=sp_model_name | TSTONEFILE=filename |
+ CITIFILE=filename] <TYPE=[s | y]>
+ <Zo=[value | vector_value]>
+ <FBASE=base_frequency> <FMAX=maximum_frequency>
+ <PRECFAC=val> <DELAYHANDLE=ON | OFF> <DELAYFREQ=val>
S Model Syntax (HSPICE RF):
.model S_model_name S
+ [FQMODEL=sp_model_name | TSTONEFILE=filename |
+ CITIFILE=filename] <TYPE=[S | Y | Z]>
+ <FBASE=base_frequency> <FMAX=max_frequency>
+ <Zo=[50 | vector_value ] | Zof=ref_model>
+ <HIGHPASS=[0 | 1 | 2]> <LOWPASS=[0 | 1 | 2]>
+ <DELAYHANDLE=[0 | 1]> <DELAYFREQ=val>
Parameter
Description
nd1 nd2 ... ndN
Nodes of an S element (see Figure 14 on page 115). Three
kinds of definitions are present:
■
With no reference node ndRef, the default reference
node in this situation is GND. Each node ndi (i=1~N) and
GND construct one of the N ports of the S element.
■
With one reference node, ndRef is defined. Each node
ndi (i=1~N) and the ndRef construct one of the N ports
of the S element.
With an N reference node, each port has its own reference
node. You can write the node definition in a clearer way as:
nd1+ nd1- nd2+ nd2- ... ndN+ ndNEach pair of the nodes (ndi+ and ndi-, i=1~N) constructs
one of the N ports of the S element.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
111
Chapter 4: Elements
Transmission Lines
Parameter
Description
nd_ref or NdR
Reference node.
MNAME
Name of the S model.
FQMODEL
Frequency behavior of the S,Y, or Z parameters. .MODEL
statement of sp type, which defines the frequency-dependent
matrices array.
TSTONEFILE
Name of a Touchstone file. Data contains frequencydependent array of matrixes. Touchstone files must follow the
.s#p file extension rule, where # represents the dimension of
the network.
For details, see Touchstone® File Format Specification by
the EIA/IBIS Open Forum (http://www.eda.org).
CITIFILE
Name of the CITIfile, which is a data file that contains
frequency-dependent data.
For details, see Using Instruments with ADS by Agilent
Technologies (http://www.agilent.com).
TYPE
Parameter type:
■
■
■
Zo
112
S (scattering), the default
Y (admittance)
Z (impedance)
Characteristic impedance value of the reference line
(frequency-independent). For multi-terminal lines (N>1),
HSPICE assumes that the characteristic impedance matrix
of the reference lines are diagonal, and their diagonal values
are set to Zo. You can also set a vector value for non-uniform
diagonal values. Use Zof to specify more general types of a
reference-line system. The default is 50.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Parameter
Description
FBASE
Base frequency used for transient analysis. HSPICE uses
this value as the base frequency point for Inverse Fast
Fourier Transformation (IFFT).
■
■
If FBASE is not set, HSPICE uses a reciprocal of the
transient period as the base frequency.
If FBASE is set smaller than the reciprocal value of
transient period, transient analysis performs circular
convolution by using the reciprocal value of FBASE as a
base period.
FMAX
Maximum frequency for transient analysis. Used as the
maximum frequency point for Inverse Fast Fourier Transform
(IFFT).
PRECFAC
Preconditioning factor to avoid a singularity (infinite
admittance matrix). See Preconditioning S Parameters on
page 117. Default=0.75.
DELAYHANDLE
Delay frequency for transmission line type parameters.
Default=OFF.
■
1 of ON activates the delay handler. See Group Delay
Handler in Time Domain Analysis on page 116
■
0 of OFF (default) deactivates the delay handler.
You must set the delay handler, if the delay of the model is
longer than the base period specified in the FBASE
parameter.
If you set DELAYHANDLE=OFF but DELAYFQ is not zero,
HSPICE simulates the S element in delay mode.
DELAYFREQ
Delay frequency for transmission-line type parameters. The
default is FMAX. If the DELAYHANDLE is set to OFF, but
DELAYFREQ is nonzero, HSPICE still simulates the S
element in delay mode.
INTERPOLATION
The interpolation method:
■
■
■
STEP: piecewise step
SPLINE: b-spline curve fit
LINEAR: piecewise linear (default)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
113
Chapter 4: Elements
Transmission Lines
Parameter
Description
INTDATTYP
Data type for the linear interpolation of the complex data.
■
■
■
HIGHPASS
RI: real-imaginary based interpolation
DBA: dB-angle based interpolation
MA: magnitude-angle based interpolation (default)
Specifies high-frequency extrapolation:
0: Use zero in Y dimension (open circuit).
1: Use highest frequency.
2: Use linear extrapolation, with the highest two points.
3: Apply window function (default).
This option overrides EXTRAPOLATION in ,model SP.
LOWPASS
Specifies low-frequency extrapolation:
0: Use zero in Y dimension (open circuit).
1: Use lowest frequency (default).
2: Use linear extrapolation, with the lowest two points.
This option overrides EXTRAPOLATION in .model SP.
MIXEDMODE
Set to 1 if the parameters are represented in the mixed mode.
DATATYPE
A string used to determine the order of the indices of the
mixed-signal incident or reflected vector. The string must be
an array of a letter and a number (Xn) where:
■
■
114
X=D to indicate a differential term
=C to indicate a common term
=S to indicate a single (grounded) term
n=the port number
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Parameter
Description
DTEMP
Temperature difference between the element and the circuit.a
Expressed in °C. The default is 0.0.
NOISE
Activates thermal noise.
■
■
1 (default): element generates thermal noise
0: element is considered noiseless
a. Circuit temperature is specified by using the .TEMP statement or by sweeping the global
TEMP variable in .DC, .AC, or .TRAN statements. When neither .TEMP or TEMP is used, circuit
temperature is set by using .OPTION TNOM. The default for TNOM is 25 °C, unless you use
.OPTION SPICE, which has a default of 27 °C. You can use the DTEMP parameter to specify
the temperature of the element.
You can set all optional parameters, except MNAME, in both the S element and
the S model statement. Parameters in element statements have higher
priorities. You must specify either the FQMODEL, TSTONEFILE, or CITIFILE
parameter in either the S model or the S element statement.
When used with the generic frequency-domain model (.MODEL SP), an S
(scattering) element is a convenient way to describe a multi-terminal network.
Figure 14
Terminal Node Notation
.
.
.
.
.
.
.
.
.
N+1 terminal system
[vinc]1
[i]1
[vinc]N
[i]N
[vref]N
[vref]1
ndN
(+) [v]N
nd1
(+) [v]1
(-)
ndR
(reference node)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
115
Chapter 4: Elements
Transmission Lines
Frequency Table Model
The frequency table model (SP model) is a generic model that you can use to
describe frequency-varying behavior. Currently, the S element and .LIN
command use this model. For a description of this model, see “Small-Signal
Parameter Data Frequency Table Model” in the HSPICE Signal Integrity User
Guide.
Group Delay Handler in Time Domain Analysis
The S element accepts a constant group delay matrix in time-domain analysis.
You can also express a weak dependence of the delay matrix on the frequency,
as a combination of the constant delay matrix and the phase shift value at each
frequency point.
To activate or deactivate this delay handler, specify the DELAYHANDLE keyword
in the S model statement.
The delay matrix is a constant matrix, which HSPICE RF extracts using finite
difference calculation at selected target frequency points. HSPICE RF obtains
the ϒ ω ( i, j ) delay matrix component as:
dθ Sij
1 dθ Sij
-----ϒ ω ( i, j ) = -------------- =
⋅ -------------2π
df
dω
■
f is the target frequency, which you can set using DELAYFREQ=val. The
default target frequency is the maximum frequency point.
■
θ Sij is the phase of Sij.
After time domain analysis obtains the group delay matrix, the following
equation eliminates the delay amount from the frequency domain systemtransfer function:
y′ mn ( ω ) = y mn ( ω ) × e
jωΤ mn
The convolution process then uses the following equation to calculate the
delay:
T
i k ( t ) = ( y′ k1 ( t ), y′ k2 ( t ), …, y′ kN ( t ) ) × ⎛ v 1 ( t – T ), v 2 ( t – T ), …, v Nt – T ⎞
⎝
⎠
K1
K2
KN
116
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 4: Elements
Transmission Lines
Preconditioning S Parameters
Certain S parameters, such as series inductor (2-port), show a singularity when
converting S to Y parameters. To avoid this singularity, the S element
preconditions S matrices by adding kRref series resistance:
S′ = [ kI + ( 2 – k )S ] [ ( 2 + k )I – kS ]
–1
■
Rref is the reference impedance vector.
■
k is the preconditioning factor.
To compensate for this modification, the S element adds a negative resistor
(-kRref) to the modified nodal analysis (NMA) matrix, in actual circuit
compensation. To specify this preconditioning factor, use the <PREFAC=val>
keyword in the S model statement. The default preconditioning factor is 0.75.
Figure 15
Preconditioning S Parameters
preconditioning
S
S
kRref
NMA stamp
kRref
Y’
Y’
Y
HSPICE® Simulation and Analysis User Guide
Y-2006.03
117
Chapter 4: Elements
IBIS Buffers
IBIS Buffers
The general syntax of a B element card for IBIS I/O buffers is:
bxxx node_1 node_2 ... node_N
+ file='filename' model='model_name'
+ keyword_1=value_1 ... [keyword_M=value_M]
Parameter
Description
bname
Buffer name, and starts with the letter B, which can be
followed by up to 1023 alphanumeric characters.
node_1 node_2 ...
node_N
List of I/O buffer external nodes. The number of nodes and
their meaning are specific to different buffer types.
file=’filename’
Name of the IBIS file.
model=’model_name’
Name of the model.
keyword_i=value_i
Assigns a value of value_i to the keyword_i keyword.
Specify optional keywords in brackets ( [ ] ). For more
information about keywords, see “Specifying Common
Keywords” in the HSPICE Signal Integrity User Guide.
Example
B1 nd_pc nd_gc nd_in nd_out_of_in
+ buffer=1
+ file='test.ibs'
+ model='IBIS_IN'
■
This example represents an input buffer named B1.
■
The four terminals are named nd_pc, nd_gc, nd_in and nd_out_of_in.
■
The IBIS model named IBIS_IN is located in the IBIS file named test.ibs.
Note:
HSPICE or HSPICE RF connects the nd_pc and nd_gc nodes to the
voltage sources. Do not manually connect these nodes to voltage
sources.
For more examples, see the “Modeling Input/Output Buffers Using IBIS”
chapter in the HSPICE Signal Integrity User Guide.
118
HSPICE® Simulation and Analysis User Guide
Y-2006.03
5
5
Sources and Stimuli
Describes element and model statements for independent sources, dependent
sources, analog-to-digital elements, and digital-to-analog elements.
This chapter also explains each type of element and model statement and
provides explicit formulas and examples to show how various combinations of
parameters affect the simulation.
Independent Source Elements
Use independent source element statements to specify DC, AC, transient, and
mixed independent voltage and current sources. Depending on the analysis
performed, the associated analysis sources are used. The value of the DC
source is overriden by the zero time value of the transient source when a
transient operating point is calculated.
Source Element Conventions
You do not need to ground voltage sources. HSPICE or HSPICE RF assumes
that positive current flows from the positive node, through the source, to the
negative node. A positive current source forces current to flow out of the n+
node, through the source, and into the n- node.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
119
Chapter 5: Sources and Stimuli
Independent Source Elements
You can use parameters as values in independent sources. Do not use any of
the following reserved keywords to identify these parameters:
AC, ACI, AM, DC, EXP, PAT, PE, PL, PU, PULSE, PWL, R, RD, SFFM, or SIN
Independent Source Element
Syntax
Vxxx n+ n- <<DC=> dcval> <tranfun> <AC=acmag> <acphase>>
Ixxx n+ n- <<DC=> dcval> <tranfun> <AC=acmag> <acphase>>
+ <M=val>
120
Parameter
Description
Vxxx
Independent voltage source element name. Must begin with V, followed
by up to 1023 alphanumeric characters.
Ixxx
Independent current source element name. Must begin with I, followed
by up to 1023 alphanumeric characters.
n+
Positive node.
n-
Negative node.
DC=dcval
DC source keyword and value, in volts. The tranfun value at time zero
overrides the DC value. Default=0.0.
tranfun
Transient source function (one or more of: AM, DC, EXP, PAT, PE, PL,
PU, PULSE, PWL, SFFM, SIN). The functions specify the
characteristics of a time-varying source. See the individual functions for
syntax.
AC
AC source keyword for use in AC small-signal analysis.
acmag
Magnitude (RMS) of the AC source, in volts.
acphase
Phase of the AC source, in degrees. Default=0.0.
M
Multiplier, to simulate multiple parallel current sources. HSPICE or
HSPICE RF multiplies source current by M. Default=1.0.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Elements
Example 1
VX 1 0 5V
Where,
■
The VX voltage source has a 5-volt DC bias.
■
The positive terminal connects to node 1.
■
The negative terminal is grounded.
Example 2
VB 2 0 DC=VCC
Where,
■
The VCC parameter specifies the DC bias for the VB voltage source.
■
The positive terminal connects to node 2.
■
The negative terminal is grounded.
Example 3
VH 3 6 DC=2 AC=1,90
Where,
■
The VH voltage source has a 2-volt DC bias, and a 1-volt RMS AC bias, with
90 degree phase offset.
■
The positive terminal connects to node 3.
■
The negative terminal connects to node 6.
Example 4
IG 8 7 PL(1MA 0S 5MA 25MS)
Where,
■
The piecewise-linear relationship defines the time-varying response for the
IG current source, which is 1 milliamp at time=0, and 5 milliamps at 25
milliseconds.
■
The positive terminal connects to node 8.
■
The negative terminal connects to node 7.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
121
Chapter 5: Sources and Stimuli
Independent Source Elements
Example 5
VCC in out VCC PWL 0 0 10NS VCC 15NS VCC 20NS 0
Where,
■
The VCC parameter specifies the DC bias for the VCC voltage source.
■
The piecewise-linear relationship defines the time-varying response for the
VCC voltage source, which is 0 volts at time=0, VCC from 10 to 15
nanoseconds, and back to 0 volts at 20 nanoseconds.
■
The positive terminal connects to the in node.
■
The negative terminal connects to the out node.
■
HSPICE or HSPICE RF determines the operating point for this source,
without the DC value (the result is 0 volts).
Example 6
VIN 13 2 0.001 AC 1 SIN (0 1 1MEG)
Where,
■
The VIN voltage source has a 0.001-volt DC bias, and a 1-volt RMS AC bias.
■
The sinusoidal time-varying response ranges from 0 to 1 volts, with a
frequency of 1 megahertz.
■
The positive terminal connects to node 13.
■
The negative terminal connects to node 2.
Example 7
ISRC 23 21 AC 0.333 45.0 SFFM (0 1 10K 5 1K)
Where,
122
■
The ISRC current source has a 1/3-amp RMS AC response, with a 45degree phase offset.
■
The frequency-modulated, time-varying response ranges from 0 to 1 volts,
with a carrier frequency of 10 kHz, a signal frequency of 1 kHz, and a
modulation index of 5.
■
The positive terminal connects to node 23.
■
The negative terminal connects to node 21.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Elements
Example 8
VMEAS 12 9
Where,
■
The VMEAS voltage source has a 0-volt DC bias.
■
The positive terminal connects to node 12.
■
The negative terminal connects to node 9.
DC Sources
For a DC source, you can specify the DC current or voltage in different ways:
V1
V1
I1
I1
1
1
1
1
0
0
0
0
DC=5V
5V
DC=5mA
5mA
■
The first two examples specify a DC voltage source of 5 V, connected
between node 1 and ground.
■
The third and fourth examples specify a 5 mA DC current source, between
node 1 and ground.
The direction of current in both sources is from node 1 to ground.
AC Sources
AC current and voltage sources are impulse functions, used for an AC analysis.
To specify the magnitude and phase of the impulse, use the AC keyword.
V1 1 0 AC=10V,90
VIN 1 0 AC 10V 90
The preceding two examples specify an AC voltage source, with a magnitude of
10 V and a phase of 90 degrees. To specify the frequency sweep range of the
AC analysis, use the .AC analysis statement. The AC or frequency domain
analysis provides the impulse response of the circuit.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
123
Chapter 5: Sources and Stimuli
Independent Source Elements
Transient Sources
For transient analysis, you can specify the source as a function of time. The
following functions are available:
■
Trapezoidal pulse (PULSE function)
■
Sinusoidal (SIN function)
■
Exponential (EXP function)
■
Piecewise linear (PWL function)
■
Single-frequency FM (SFFM function)
■
Single-frequency AM (AM function)
■
Pattern (PAT function)
Pseudo Random-Bit Generator Source (PRBS function)
Mixed Sources
Mixed sources specify source values for more than one type of analysis. For
example, you can specify a DC source, an AC source, and a transient source,
all of which connect to the same nodes. In this case, when you run specific
analyses, HSPICE or HSPICE RF selects the appropriate DC, AC, or transient
source. The exception is the zero-time value of a transient source, which overrides the DC value; it is selected for operating-point calculation for all analyses.
Example
VIN 13 2 0.5 AC 1 SIN (0 1 1MEG)
Where,
■
DC source of 0.5 V
■
AC source of 1 V
■
Transient damped sinusoidal source
Each source connects between nodes 13 and 2.
For DC analysis, the program uses zero source value, because the sinusoidal
source is zero at time zero.
124
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Elements
Port Element
The port element identifies the ports used in .LIN analysis. Each port element
requires a unique port number. If your design uses N port elements, your netlist
must contain the sequential set of port numbers, 1 through N (for example, in a
design containing 512 ports, you must number each port sequentially, 1 to
512).
Each port has an associated system impedance, zo. If you do not explicitly
specify the system impedance, the default is 50 ohms.
The port element behaves as either a noiseless impedance or a voltage source
in series with the port impedance for all other analyses (DC, AC, or TRAN).
■
You can use this element as a pure terminating resistance or as a voltage or
power source.
■
You can use the RDC, RAC, RHB, RHBAC, and rtran values to override the port
impedance value for a particular analysis.
Syntax
Pxxx p n port=portnumber
+ $ **** Voltage or Power Information ********
+ <DC mag> <AC <mag <phase>>> <HBAC <mag <phase>>>
+ <HB <mag <phase <harm <tone <modharm <modtone>>>>>>>
+ <transient_waveform> <TRANFORHB=[0|1]>
+ <DCOPEN=[0|1]>
+ $ **** Source Impedance Information ********
+ <Z0=val> <RDC=val> <RAC=val>
+ <RHBAC=val> <RHB=val> <RTRAN=val>
+ $ **** Power Switch ********
+ <power=[0|1|2|W|dbm]>
Parameter
Description
port=portnumber
The port number. Numbered sequentially beginning
with 1 with no shared port numbers.
<DC mag>
DC voltage or power source value.
<AC <mag <phase>>>
AC voltage or power source value.
<HBAC <mag <phase>>>
(HSPICE RF) HBAC voltage or power source value.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
125
Chapter 5: Sources and Stimuli
Independent Source Elements
Parameter
Description
<HB <mag <phase <harm
<tone <modharm
<modtone>>>>>>>
(HSPICE RF) HB voltage, current, or power source
value. Multiple HB specifications with different harm,
tone, modharm, and modtone values are allowed.
■
■
■
<transient_waveform>
126
phase is in degrees
harm and tone are indices corresponding to the
tones specified in the .HB statement. Indexing starts
at 1 (corresponding to the first harmonic of a tone).
modtone and modharm specify sources for multitone simulation. A source specifies a tone and a
harmonic, and up to 1 offset tone and harmonic
(modtone for tones and modharm for harmonics).
The signal is then described as:
V(or I)=mag*cos(2*pi*
(harm*tone+modharm*modtone)*t + phase)
(Transient analysis) Voltage or power source waveform.
Any one of waveforms: AM, EXP, PULSE, PWL, SFFM,
SIN, or PRBS. Multiple transient descriptions are not
allowed.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Elements
Parameter
Description
<TRANFORHB=[0|1]>
■
0 (default): The transient description is ignored if an
HB value is given or a DC value is given. If no DC or
HB value is given and TRANFORHB=0, then HB
analysis treats the source as a DC source, and the
DC source value is the time=0 value.
■
1: HB analysis uses the transient description if its
value is VMRF, SIN, PULSE, PWL, or LFSR. If the
type is a non-repeating PWL source, then the
time=infinity value is used as a DC analysis source
value. For example, the following statement is treated
as a DC source with value=1 for HB analysis:
v1 1 0 PWL (0 0 1n 1 1u 1)
+ TRANFORHB=1
In contrast, the following statement is a 0V DC
source:
v1 1 0 PWL (0 0 1n 1 1u 1)
+ TRANFORHB=0
The following statement is treated as a periodic
source with a 1us period that uses PWL values:
v1 1 0 PWL (0 0 1n 1 0.999u 1 1u 0) R
+ TRANFORHB=1
To override the global TRANFORHB option, explicitly
set TRANFORHB for a voltage or current source.
DCOPEN
Switch for open DC connection when DC mag is not set.
■
■
<z0=val>
0 (default): P element behaves as an impedance
termination.
1 : P element is considered an open circuit in DC
operating point analysis. DCOPEN=1 is mainly used
in .LIN analysis so the P element will not affect the
self-biasing device under test by opening the
termination at the operating point.
(LIN analysis) System impedance used when
converting to a power source, inserted in series with the
voltage source. Currently, this only supports real
impedance.
■
When power=0, z0 defaults to 0.
When power=1, z0 defaults to 50 ohms.
You can also enter zo=val.
■
HSPICE® Simulation and Analysis User Guide
Y-2006.03
127
Chapter 5: Sources and Stimuli
Independent Source Elements
Parameter
Description
<RDC=val>
(DC analysis) Series resistance (overrides z0).
<RAC=val>
(AC analysis) Series resistance (overrides z0).
<RHBAC=val>
(HSPICE RF HBAC analysis) Series resistance
(overrides z0).
<RHB=val>
(HSPICE RF HB analysis) Series resistance (overrides
z0).
<RTRAN=val>
(Transient analysis) Series resistance (overrides z0).
<power=[0 | 1 | 2 | W | dbm]> (HSPICE RF) power switch
■
When 0 (default), element treated as a voltage or
current source.
■
When 1 or W, element treated as a power source,
realized as a voltage source with a series
impedance. In this case, the source value is
interpreted as RMS available power in units of Watts.
■
When 2 or dbm, element treated as a power source
in series with the port imedance. Values are in dbms.
You can use this parameter for transient analysis if the
power source is either DC or SIN.
Example
For example, the following port element specifications identify a 2-port network
with 50-Ohm reference impedances between the "in" and "out" nodes.
P1 in gnd port=1 z0=50
P2 out gnd port=2 z0=50
Computing scattering parameters requires z0 reference impedance values.
The order of the port parameters (in the P Element) determines the order of the
S, Y, and Z parameters. Unlike the .NET command, the .LIN command does
not require you to insert additional sources into the circuit. To calculate the
requested transfer parameters, HSPICE automatically inserts these sources as
needed at the port terminals. You can define an unlimited number of ports.
128
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Independent Source Functions
HSPICE or HSPICE RF uses the following types of independent source
functions:
■
Trapezoidal pulse (PULSE function)
■
Sinusoidal (SIN function)
■
Exponential (EXP function)
■
Piecewise linear (PWL function)
■
Single-frequency FM (SFFM function)
■
Single-frequency AM (AM function)
■
Pattern (PAT function)
Pseudo Random-Bit Generator Source (PRBS function)
HSPICE also provides a data-driven version of PWL (not supported in HSPICE
RF). If you use the data-driven PWL, you can reuse the results of an experiment
or of a previous simulation, as one or more input sources for a transient
simulation.
If you use the independent sources supplied with HSPICE or HSPICE RF, you
can specify several useful analog and digital test vectors for steady state, time
domain, or frequency domain analysis. For example, in the time domain, you
can specify both current and voltage transient waveforms, as exponential,
sinusoidal, piecewise linear, AM, or single-sided FM functions.
Trapezoidal Pulse Source
HSPICE or HSPICE RF provides a trapezoidal pulse source function, which
starts with an initial delay from the beginning of the transient simulation interval,
to an onset ramp. During the onset ramp, the voltage or current changes
linearly, from its initial value, to the pulse plateau value. After the pulse plateau,
the voltage or current moves linearly, along a recovery ramp, back to its initial
value. The entire pulse repeats, with a period named per, from onset to onset.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
129
Chapter 5: Sources and Stimuli
Independent Source Functions
Syntax
Vxxx n+ n- PU<LSE> <(>v1 v2 <td <tr <tf <pw <per>>>>> <)>
Ixxx n+ n- PU<LSE> <(>v1 v2 <td <tr <tf <pw + <per>>>>> <)>
Parameter
Description
Vxxx, Ixxx
Independent voltage source, which exhibits the pulse response.
PULSE
Keyword for a pulsed time-varying source. The short form is PU.
v1
Initial value of the voltage or current, before the pulse onset (units of
volts or amps).
v2
Pulse plateau value (units of volts or amps).
td
Delay (propagation) time in seconds, from the beginning of the
transient interval, to the first onset ramp. Default=0.0; HSPICE or
HSPICE RF sets negative values to zero.
tr
Duration of the onset ramp (in seconds), from the initial value, to the
pulse plateau value (reverse transit time). Default=TSTEP.
tf
Duration of the recovery ramp (in seconds), from the pulse plateau,
back to the initial value (forward transit time). Default=TSTEP.
pw
Pulse width (the width of the plateau portion of the pulse), in
seconds. Default=TSTOP.
per
Pulse repetition period, in seconds. Default=TSTOP.
Table 8
130
Time-Value Relationship for a PULSE Source
Time
Value
0
v1
td
v1
td + tr
v2
td + tr + pw
v2
td + tr + pw + tf
v1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Table 8
Time-Value Relationship for a PULSE Source (Continued)
Time
Value
tstop
v1
Linear interpolation determines the intermediate points.
Note:
TSTEP is the printing increment, and TSTOP is the final time.
Example 1
The following example shows the pulse source, connected between node 3 and
node 0. In the pulse:
■
The output high voltage is 1 V.
■
The output low voltage is -1 V.
■
The delay is 2 ns.
■
The rise and fall time are each 2 ns.
■
The high pulse width is 50 ns.
■
The period is 100 ns.
VIN 3 0 PULSE (-1 1 2NS 2NS 2NS 50NS 100NS)
Example 2
The following example is a pulse source, which connects between node 99 and
node 0. The syntax shows parameter values for all specifications.
V1 99 0 PU lv hv tdlay tris tfall tpw tper
Example 3
The following example shows an entire netlist, which contains a PULSE voltage
source. In the source:
■
The initial voltage is 1 volt.
■
The pulse voltage is 2 volts.
■
The delay time, rise time, and fall time are each 5 nanoseconds.
■
The pulse width is 20 nanoseconds.
■
The pulse period is 50 nanoseconds.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
131
Chapter 5: Sources and Stimuli
Independent Source Functions
This example is based on demonstration netlist pulse.sp, which is available in
directory $<installdir>/demo/hspice/sources:
file pulse.sp test of pulse
.option post
.tran .5ns 75ns
vpulse 1 0 pulse( v1 v2 td tr tf pw per )
r1 1 0 1
.param v1=1v v2=2v td=5ns tr=5ns tf=5ns pw=20ns per=50ns
.end
Figure 16 shows the result of simulating this netlist, in HSPICE or HSPICE RF.
Figure 16
132
Pulse Source Function
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Sinusoidal Source Function
HSPICE or HSPICE RF provides a damped sinusoidal source funtion, which is
the product of a dying exponential with a sine wave. To apply this waveform,
you must specify:
■
Sine wave frequency
■
Exponential decay constant
■
Beginning phase
■
Beginning time of the waveform
Syntax
Vxxx n+ n- SIN <(> vo va <freq <td <q <j>>>> <)>
Ixxx n+ n- SIN <(> vo va <freq <td <q <j>>>> <)>
Parameter
Description
Vxxx, Ixxx
Independent voltage source that exhibits the sinusoidal response.
SIN
Keyword for a sinusoidal time-varying source.
vo
Voltage or current offset, in volts or amps.
va
Voltage or current peak value (vpeak), in volts or amps.
freq
Source frequency in Hz. Default=1/TSTOP.
td
Time (propagation) delay before beginning the sinusoidal variation, in
seconds. Default=0.0. Response is 0 volts or amps, until HSPICE or
HSPICE RF reaches the delay value, even with a non-zero DC voltage.
q
Damping factor, in units of 1/seconds. Default=0.0.
j
Phase delay, in units of degrees. Default=0.0.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
133
Chapter 5: Sources and Stimuli
Independent Source Functions
The following table of expressions defines the waveform shape:
Table 9
Waveform Shape Expressions
Time
Value
0 to td
td to tstop
2⋅Π⋅ϕ
vo + va ⋅ SIN ⎛⎝ --------------------⎞⎠
360
vo + va ⋅ Exp [ – ( Time – td ) ⋅ θ ]
ϕ ⎫
⎧
SIN ⎨ 2 ⋅ Π ⋅ freq ⋅ ( time – td ) + --------- ⎬
360
⎩
⎭
In these expressions, TSTOP is the final time.
Example
VIN 3 0 SIN (0 1 100MEG 1NS 1e10)
This damped sinusoidal source connects between nodes 3 and 0. In this
waveform:
■
Peak value is 1 V.
■
Offset is 0 V.
■
Frequency is 100 MHz.
■
Time delay is 1 ns.
■
Damping factor is 1e10.
■
Phase delay is zero degrees.
See Figure 17 on page 135 for a plot of the source output.
134
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Figure 17
Sinusoidal Source Function
This example is based on demonstration netlist sin.sp, which is available in
directory $<installdir>/demo/hspice/sources:
*file: sin.spsinusoidal source
.options post
.param v0=0 va=1 freq=100meg delay=2n theta=5e7 phase=0
v 1 0 sin(v0 va freq delay theta phase)
r 1 0 1
.tran .05n 50n
.end
HSPICE® Simulation and Analysis User Guide
Y-2006.03
135
Chapter 5: Sources and Stimuli
Independent Source Functions
Table 10
SIN Voltage Source
Parameter
Value
initial voltage
0 volts
pulse voltage
1 volt
delay time
2 nanoseconds
frequency
100 MHz
damping factor
50 MHz
Exponential Source Function
HSPICE or HSPICE RF provides a exponential source function, in an
independent voltage or current source.
Syntax
Vxxx n+ n- EXP <(> v1 v2 <td1 <t1 <td2 <t2>>>> <)>
Ixxx n+ n- EXP <(> v1 v2 <td1 <t1 <td2 <t2>>>> <)>
136
Parameter
Description
Vxxx, Ixxx
Independent voltage source, exhibiting an exponential response.
EXP
Keyword for an exponential time-varying source.
v1
Initial value of voltage or current, in volts or amps.
v2
Pulsed value of voltage or current, in volts or amps.
td1
Rise delay time, in seconds. Default=0.0.
td2
Fall delay time, in seconds. Default=td1+TSTEP.
t1
Rise time constant, in seconds. Default=TSTEP.
t2
Fall time constant, in seconds. Default=TSTEP.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
TSTEP is the printing increment, and TSTOP is the final time.
The following table of expressions defines the waveform shape:
Table 11
Waveform Shape Definitions
Time
Value
0 to td1
v1
td1 to td2
– td1⎞
v1 + ( v2 – v1 ) ⋅ 1 – exp ⎛ – Time
-⎠
⎝ -------------------------τ
1
td2 to tstop
Time – td1 )-⎞ +
v1 + ( v2 – v1 ) ⋅ 1 – exp ⎛ – (------------------------------⎝
⎠
τ
1
( Time – td2 -)⎞
( v1 – v2 ) ⋅ 1 – exp ⎛⎝ – ------------------------------⎠
τ2
Example
VIN 3 0 EXP (-4 -1 2NS 30NS 60NS 40NS)
The above example describes an exponential transient source, which connects
between nodes 3 and 0. In this source:
■
Initial t=0 voltage is -4 V.
■
Final voltage is -1 V.
■
Waveform rises exponentially, from -4 V to -1 V, with a time constant of 30
ns.
■
At 60 ns, the waveform starts dropping to -4 V again, with a time constant of
40 ns.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
137
Chapter 5: Sources and Stimuli
Independent Source Functions
Figure 18
Exponential Source Function
This example is based on demonstration netlist exp.sp, which is available in
directory $<installdir>/demo/hspice/sources:
*file: exp.spexponential independant source
.options post
.param v0=-4 va=-1 td1=5n tau1=30n tau2=40n td2=80n
v 1 0 exp(v0 va td1 tau1 td2 tau2)
r 1 0 1
.tran .05n 200n
.end
This example shows an entire netlist, which contains an EXP voltage source. In
this source:
138
■
Initial t=0 voltage is -4 V.
■
Final voltage is -1 V.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
■
Waveform rises exponentially, from -4 V to -1 V, with a time constant of 30
ns.
■
At 80 ns, the waveform starts dropping to -4 V again, with a time constant of
40 ns.
Piecewise Linear Source
HSPICE or HSPICE RF provides a piecewise linear source function, in an
independent voltage or current source.
General Form
Vxxx n+ n- PWL <(> t1 v1 <t2 v2 t3 v3…> <R <=repeat>>
+ <TD=delay> <)>
Ixxx n+ n- PWL <(> t1 v1 <t2 v2 t3 v3…> <R <=repeat>>
+ <TD=delay> <)>
MSINC and ASPEC Form
Vxxx n+ n- PL <(> v1 t1 <v2 t2 v3 t3…> <R <=repeat>>
+ <TD=delay> <)>
Ixxx n+ n- PL <(> v1 t1 <v2 t2 v3 t3…> <R <=repeat>>
+ <TD=delay> <)>
Parameter
Description
Vxxx, Ixxx
Independent voltage source; uses a piecewise linear response.
PWL
Keyword for a piecewise linear time-varying source.
v1 v2 … vn
Current or voltage values at the corresponding timepoint.
t1 t2 … tn
Timepoint values, where the corresponding current or voltage value is
valid.
R=repeat
Keyword and time value to specify a repeating function. With no
argument, the source repeats from the beginning of the function.
repeat is the time, in units of seconds, which specifies the start point
of the waveform to repeat. This time needs to be less than the greatest
time point, tn.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
139
Chapter 5: Sources and Stimuli
Independent Source Functions
Parameter
Description
TD=delay
Time, in units of seconds, which specifies the length of time to delay
(propagation delay) the piecewise linear function.
■
Each pair of values (t1, v1) specifies that the value of the source is v1 (in
volts or amps), at time t1.
■
Linear interpolation between the time points determines the value of the
source, at intermediate values of time.
■
The PL form of the function accommodates ASPEC style formats, and
reverses the order of the time-voltage pairs to voltage-time pairs.
■
If you do not specify a time-zero point, HSPICE or HSPICE RF uses the DC
value of the source, as the time-zero source value.
HSPICE or HSPICE RF does not force the source to terminate at the TSTOP
value, specified in the .TRAN statement.
If the slope of the piecewise linear function changes below a specified
tolerance, the timestep algorithm might not choose the specified time points as
simulation time points. To obtain a value for the source voltage or current,
HSPICE or HSPICE RF extrapolates neighboring values. As a result, the
simulated voltage might deviate slightly from the voltage specified in the PWL
list. To force HSPICE or HSPICE RF to use the specified values, use .OPTION
SLOPETOL, which reduces the slope change tolerance.
R causes the function to repeat. You can specify a value after this R, to indicate
the beginning of the function to repeat. The repeat time must equal a
breakpoint in the function. For example, if t1=1, t2=2, t3=3, and t4=4, then the
repeat value can be 1, 2, or 3.
Specify TD=val to cause a delay at the beginning of the function. You can use
TD with or without the repeat function.
140
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Example
This example is based on demonstration netlist pwl.sp, which is available in
directory $<installdir>/demo/hspice/sources:
file pwl.sp repeated piecewise linear source
.option post
.tran 5n 500n
v1 1 0 pwl 60n 0v, 120n 0v, 130n 5v, 170n 5v, 180n 0v, r
r1 1 0 1
v2 2 0 pl 0v 60n, 0v 120n, 5v 130n, 5v 170n, 0v 180n, r 60n
r2 2 0 1
.end
This example shows an entire netlist, which contains two piecewise linear
voltage sources. The two sources have the same function:
■
First is in normal format. The repeat starts at the beginning of the function.
■
Second is in ASPEC format. The repeat starts at the first timepoint.
See Figure 19 for the difference in responses.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
141
Chapter 5: Sources and Stimuli
Independent Source Functions
Figure 19
Results of Using the Repeat Function
Data-Driven Piecewise Linear Source
HSPICE provides a data-driven piecewise linear source function, in an
independent voltage or current source.
Syntax
Vxxx n+ n- PWL (TIME, PV)
Ixxx n+ n- PWL (TIME, PV)
.DATA dataname
TIME PV
t1 v1
t2 v2
t3 v3
t4 v4
. . . .
.ENDDATA
.TRAN DATA=datanam
142
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Parameter
Description
TIME
Parameter name for time value, provided in a .DATA statement.
PV
Parameter name for amplitude value, provided in a .DATA statement.
You must use this source with a .DATA statement that contains time-value
pairs. For each tn-vn (time-value) pair that you specify in the .DATA block, the
data-driven PWL function outputs a current or voltage of the specified tn
duration and with the specified vn amplitude.
When you use this source, you can reuse the results of one simulation, as an
input source in another simulation. The transient analysis must be data-driven.
Example
This example is based on demonstration netlist datadriven_pwl.sp, which is
available in directory $<installdir>/demo/hspice/sources:
*DATA DRIVEN PIECEWISE LINEAR SOURCE
.options list node post
V1 1 0 PWL(TIME, pv1)
R1 1 0 1
V2 2 0 PWL(TIME, pv2)
R2 2 0 1
.DATA dsrc
TIME pv1 pv2
0n 5v 0v
5n 0v 5v
10n 0v 5v
.ENDDATA
.TRAN 1p 10n sweep DATA=dsrc
.END
This example is an entire netlist, containing two data-driven, piecewise linear
voltage sources. The .DATA statement contains the two sets of values
referenced in the pv1 and pv2 sources. The .TRAN statement references the
data name.
Single-Frequency FM Source
HSPICE or HSPICE RF provides a single-frequency FM source function, in an
independent voltage or current source.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
143
Chapter 5: Sources and Stimuli
Independent Source Functions
Syntax
Vxxx n+ n- SFFM <(> vo va <fc <mdi <fs>>> <)>
Ixxx n+ n- SFFM <(> vo va <fc <mdi <fs>>> <)>
Parameter
Description
Vxxx, Ixxx
Independent voltage source, which exhibits the frequencymodulated response.
SFFM
Keyword for a single-frequency, frequency-modulated, time-varying
source.
vo
Output voltage or current offset, in volts or amps.
va
Output voltage or current amplitude, in volts or amps.
fc
Carrier frequency, in Hz. Default=1/TSTOP.
mdi
Modulation index, which determines the magnitude of deviation from
the carrier frequency. Values normally lie between 1 and 10.
Default=0.0.
fs
Signal frequency, in Hz. Default=1/TSTOP.
The following expression defines the waveform shape:
sourcevalue = vo + va ⋅ SIN [ 2 ⋅ π ⋅ fc ⋅ Time + mdi ⋅ SIN ( 2 ⋅ π ⋅ fs ⋅ Time ) ]
Example
This example is based on demonstration netlist sffm.sp, which is available in
directory $<installdir>/demo/hspice/sources:
*file: sffm.spfrequency modulation source
.options post
vsff1 15 0 dc 3v sffm(0v 1v 20k 10 5k)
rssf1 15 0 1
.tran .001ms .5ms
.probe tran v(15)
.end
This example shows an entire netlist, which contains a single-frequency,
frequency-modulated voltage source. In this source.
144
■
The offset voltage is 0 volts.
■
The maximum voltage is 1 millivolt.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
■
The carrier frequency is 20 kHz.
■
The signal is 5 kHz, with a modulation index of 10 (the maximum wavelength
is roughly 10 times as long as the minimum).
Figure 20
Single Frequency FM Source
Single-Frequency AM Source
HSPICE or HSPICE RF provides a single-frequency AM source function in an
independent voltage or current source.
Syntax
Vxxx n+ n- AM < (> sa oc fm fc <td> <)>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
145
Chapter 5: Sources and Stimuli
Independent Source Functions
Ixxx n+ n- AM < (> sa oc fm fc <td> <)>
Parameter
Description
Vxxx, Ixxx
Independent voltage source, which exhibits the amplitude-modulated
response.
AM
Keyword for an amplitude-modulated, time-varying source.
sa
Signal amplitude, in volts or amps. Default=0.0.
fc
Carrier frequency, in hertz. Default=0.0.
fm
Modulation frequency, in hertz. Default=1/TSTOP.
oc
Offset constant, a unitless constant that determines the absolute
magnitude of the modulation. Default=0.0.
td
Delay time (propagation delay) before the start of the signal, in seconds.
Default=0.0.
The following expression defines the waveform shape:
sourcevalue = sa ⋅ { oc + SIN [ 2 ⋅ π ⋅ fm ⋅ ( Time – td ) ] } ⋅ SIN [ 2 ⋅ π ⋅ fc ⋅ ( Time – td ) ]
Example
This example is based on demonstration netlist amsrc.sp, which is available in
directory $<installdir>/demo/hspice/sources:
*file amsrc.sp amplitude modulation
.option post
.tran .01m 20m
v1 1 0 am(10 1 100 1k 1m)
r1 1 0 1
v2 2 0 am(2.5 4 100 1k 1m)
r2 2 0 1
v3 3 0 am(10 1 1k 100 1m)
r3 3 0 1
.end
This example shows an entire netlist, which contains three amplitudemodulated voltage sources.
146
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
■
■
■
In the first source:
•
Amplitude is 10.
•
Offset constant is 1.
•
Carrier frequency is 1 kHz.
•
Modulation frequency of 100 Hz.
•
Delay is 1 millisecond.
In the second source, only the amplitude and offset constant differ from the
first source:
•
Amplitude is 2.5.
•
Offset constant is 4.
•
Carrier frequency is 1 kHz.
•
Modulation frequency of 100 Hz.
•
Delay is 1 millisecond.
The third source exchanges the carrier and modulation frequencies,
compared to the first source:
•
Amplitude is 10.
•
Offset constant is 1.
•
Carrier frequency is 100 Hz.
•
Modulation frequency of 1 kHz.
•
Delay is 1 millisecond.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
147
Chapter 5: Sources and Stimuli
Independent Source Functions
Figure 21
Amplitude Modulation Plot
Pattern Source
HSPICE or HSPICE RF provides a pattern source function, in an independent
voltage or current source. The pattern source function uses four states,
'1','0','m', and 'z', which represent the high, low, middle voltage, or current and
high impedance state respectively. The series of these four states is called a “bstring.”
Syntax
Vxxx n+ n- PAT <(> vhi vlo td tr tf
+ <R=repeat> <)>
Ixxx n+ n- PAT <(> vhi vlo td tr tf
+ <R=repeat> <)>
148
tsample data <RB=val>
tsample data <RB=val>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Parameter
Description
Vxxx, Ixxx
Independent voltage source that exhibits a pattern response.
PAT
Keyword for a pattern time-varying source.
vhi
High voltage or current value for pattern sources (units of volts
or amps).
vlo
Low voltage or current value for pattern sources (units of volts
or amps).
td
Delay (propagation) time in seconds from the beginning of the
transient interval to the first onset ramp. It can be negative. The
state in the delay time is the same as the first state specified in
data.
tr
Duration of the onset ramp (in seconds) from the low value to
the high value (reverse transit time).
tf
Duration of the recovery ramp (in seconds) from the high value
back to the low value (forward transit time).
tsample
Time spent at '0' or '1' or 'M' or 'Z' pattern value (in seconds).
data
String of '1' ,'0','M', 'Z' representing a pattern source. The first
alphabet must be 'B', which represents it is a binary bit stream.
This series is called b-string. '1' represents the high voltage or
current value, '0' is the low voltage or current value, 'M'
represents the value which is equal to 0.5*(vhi+vlo).'Z'
represents the high impedance state (only for voltage source).
RB
Keyword to specify the starting bit when repeating. The repeat
data starts from the bit indicated by RB. RB must be an integer.
If the value is larger than the length of the b-string, an error is
reported. If the value is less than 1, it is set to 1 automatically.
R=repeat
Keyword to specify how many times to execute the repeating
operation be executed. With no argument, the source repeats
from the beginning of the b-string. If R=-1, it means the
repeating operation will continue forever. R must be an integer
and if it is less than -1, it will be set to 0 automatically.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
149
Chapter 5: Sources and Stimuli
Independent Source Functions
The time from 0 to the first transition is:
tdelay+N*tsample-tr(tf)/2
■
N is the number of the same bit, from the beginning.
■
If the first transition is rising, this equation uses tr.
■
If the first transition is falling, it uses tf.
Example
The following example shows a pattern source with two b-strings:
*FILE: pattern source gereral form
v1 1 0 pat (5 0 0n 1n 1n 5n b1011 r=1 rb=2 b0m1z)
r1 1 0 1
In this pattern:
■
High voltage is 5 v
■
Low voltage is 0 v
■
Time delay is 0 n
■
Rise time is 1 n
■
Fall time is 1 n
■
Sample time is 5 n
The first b-string is 1011, which repeats once and then repeats from the
second bit, which is 0. The second b-string is 0m1z. Since neither R and RB is
specified here, they are set to the default value, which is R=0, RB=1.
Example
The following b-string and its repeat time R and repeating start bit RB cannot
use a parameter—it is considered as a undivided unit in HSPICE and can only
be defined in a .PAT command.
*FILE:pattern source using parameter
.param td=40ps tr=20ps tf=80ps tsample=400ps
VIN 1 0 PAT (2 0 td tr tf tsample b1010110 r=2)
r1 1 0 1
In this pattern:
150
■
High voltage is 2 V.
■
Low voltage is 0 V.
■
Time delay is 40 ps.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
■
Rise time is 20 ps.
■
Fall time is 80 ps.
■
Sample time is 400 ps.
■
Data is 1010110.
Nested-Structure Pattern Source HSPICE provides Nested Structure (NS)
for the pattern source function to construct complex waveforms. NS is a
combination of a b-string and other nested structures defined in a .PAT
command, which is explained later in this section.
The following general syntax is for an NS pattern source.
Syntax
Vxxx n+ n- PAT
+ [component 1
Ixxx n+ n- PAT
+ [component 1
<(>
...
<(>
...
vhi vlo td tr tf tsample
component n] <RB=val> <R=repeat> <)>
vhi vlo td tr tf tsample
component n] <RB=val> <R=repeat> <) >
Parameter
Description
component
Component is the element that makes up NS, which can be
a b-string or a patname defined in other PAT commands.
Brackets ( [ ] ) must be used.
RB=val
Keyword to specify the starting component when
repeating. The repeat data starts from the component
indicated by RB. RB must be an integer. If RB is larger than
the length of the NS, an error is reported. If RB is less than
1, it is automatically set to 1.
R=repeat
Keyword to specify how many times the repeating
operation is executed. With no argument, the source
repeats from the beginning of the NS. If R=-1, the repeating
operation continuse forever. R must be an integer, and if it
is less than -1, it is automatically set to 0.
If the component is a b-string, it can also be followed by R=repeat and
RB=val to specify the repeat time and repeating start bit.
Example
*FILE: Pattern source using nested structure
v1 1 0 pat (5 0 0n 1n 1n 5n [b1011 r=1 rb=2 b0m1z] r=2 rb=2)
r1 1 0 1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
151
Chapter 5: Sources and Stimuli
Independent Source Functions
When expanding the nested structure, you get the pattern source like this:
'b1011 r=1 rb=2 b0m1z b0m1z b0m1z'
The whole NS repeats twice, and each time it repeats from the second b0m1z
component.
Pattern-Command Driven Pattern Source The following general syntax is
for including a pattern-command driven pattern source in an independent
voltage or current source. The RB and R of a b-string or NS can be reset in an
independent source. With no argument, the R and RB are the same when
defined in the pattern command.
Syntax
Vxxx n+ n- PAT <(> vhi vlo td tr tf tsample PatName <RB=val>
+ <R=repeat> <)>
Ixxx n+ n- PAT <(> vhi vlo td tr tf tsample Patname <RB=val>
+ <R=repeat> <)>
Additional syntax applies to the .PAT-command driven pattern source:
.PAT <PatName>=data <RB=val> <R=repeat>
.PAT <patName>=[component 1 ... component n] <RB=val>
<R=repeat>
The PatName is the pattern name that has an associated b-string or nested
structure.
Example 1
v1 1 0 pat (5 0 0n 1n 1n 5n a1 a2 r=2 rb=2)
.PAT a1=b1010 r=1 rb=1
.PAT a2=b0101 r=1 rb=1
The final pattern source is:
b1010 r=1 rb=1 b0101 r=2 rb=2
When the independent source uses the pattern command to specify its pattern
source, r and rb can be reset.
Example 2
*FILE 2: Pattern source driven by pattern command
v1 1 0 pat (5 0 0n 1n 1n 5n [a1 b0011] r=1 rb=1)
.PAT a1=[b1010 b0101] r=0 rb=1
152
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
The final pattern source is:
b1010 b0101 b0011 b1010 b0101 b0011
The a1 is a predefined NS, and it can be referenced by pattern source.
Pseudo Random-Bit Generator Source
HSPICE or HSPICE RF Pseudo Random Bit Generator Source (PRBS)
function, in an independent voltage or current source. This function can be
used in several applications from cryptography and bit-error-rate measurement,
to wireless communication systems employing spread spectrum or CDMA
techniques. In general, PRBS uses a Linear Feedback Shift Register (LFSR) to
generate a pseudo random bit sequence.
Syntax
Vxxx n+ n- LFSR <(> vlow vhigh tdelay trise tfall rate seed <[>
+ taps <]> <rout=val> <)>
Ixxx n+ n- LFSR <(> vlow vhigh tdelay trise tfall rate seed <[>
+ taps <]> <rout=val> <)>
Parameter Description
LFSR
Specifies the voltage or current source as PRBS.
vlow
The minimum voltage or current level.
vhigh
The maximum voltage or current level.
tdelay
Specifies the initial time delay to the first transition.
trise
Specifies the duration of the onset ramp (in seconds), from the initial value
to the pulse plateau value (reverse transit time).
tfall
Specifies the duration of the recovery ramp (in seconds), from the pulse
plateau, back to the initial value (forward transit time).
rate
The bit rate.
seed
The initial value loaded into the shift register.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
153
Chapter 5: Sources and Stimuli
Independent Source Functions
Parameter Description
taps
The bits used to generate feedback.
rout
The output resistance.
Example 1
The following example shows the pattern source that is connected between
node in and node gnd:
vin in gnd LFSR (0 1 1m 1n 1n 10meg 1 [5, 2] rout=10)
Where,
■
The output low voltage is 0 , and the output high voltage is 1 v.
■
The delay time is 1 ms.
■
The rise and fall times are each 1 ns.
■
The bit rate is 10meg bits/s.
■
The seed is 1.
■
The taps are [5, 2].
■
The output resistance is 10 ohm.
■
The output from the LFSR is: 1000010101110110001111100110100...
Example 2
The following example shows the pattern source connected between node 1
and node 0:
.PARAM td1=2.5m tr1=2n
vin 1 0 LFSR (2 4 td1 tr1 1n 6meg 2 [10, 5, 3, 2])
Where,
154
■
The output low voltage is 2 v, and the output high voltage is 4 v.
■
The delay is 2.5 ms.
■
The rise time is 2 ns, and the fall time is 1 ns.
■
The bit rate is 6meg bits/s.
■
The seed is 2.
■
The taps are [10, 5, 3, 2].
■
The output resistance is 0 ohm.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Independent Source Functions
Example 3
This example is based on demonstration netlist prbs.sp, which is available in
directory $<installdir>/demo/hspice/sources:
* prbs.sp
.OPTION POST
.TRAN 0.5n 50u
V1 1 0 LFSR (0 1 1u 1n 1n 10meg 1 [5, 2] rout=10)
R1 1 0 1
.END
Linear Feedback Shift Register
A LFSR consists of several simple-shift registers in which a binary-weighted
modulo-2 sum of the taps is fed back to the input. The modulo-2 sum of two1bit binary numbers yields 0 if the two numbers are identical and 1 if the differ is
0+0=0, 0+1=1, or 1+1=0.
Figure 22
LFSR Diagram
g(0)
g(1)
g(2)
g(m-1)
g(m)
D(n)
input
D(n-1)
D(n-2)
D(2)
D(1)
output
For any given tap, the weight “gi” is either 0, (meaning "no connection"), or 1,
(meaning it is fed back). Two exceptions are g0 and gm, which are always 1
and therefore always connected. The gm is not really a feedback connection,
but rather an input of the shift register that is assigned a feedback weight for
mathematical purposes.
The maximum number of bits is defined by the first number in your TAPS
definition. For example [23, 22, 21, 20, 19, 7] denotes a 23 stage LFSR. The
TAPS definition is a specific feedback tap sequence that generates an
M-Sequence PRB. The LFSR stages limit is between 2 and 30. The seed
cannot be set to zero; HSPICE reports an error and exits the simulation if you
set the seed to zero.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
155
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
Conventions for Feedback Tap Specification
A given set of feedback connections can be expressed in a convenient and
easy-to-use shorthand form with the connection numbers listed within a pair of
brackets. The g0 connection is implied and not listed since it is always
connected. Although gm is also always connected, it is listed in order to convey
the shift register size (number of registers).
The following line is a set of feedback taps where j is the total number of
feedback taps (not including g0), f(1)=m is the highest-order feedback tap (and
the size of the LFSR), and f(j) are the remaining feedback taps:
[f(1), f(2), f(3), ..., f(j)]
Example
The following line shows that the number of registers is 7 and the total number
of feedback taps is 4:
[7, 3, 2, 1]
The following feedback input applies for this specification:
D(n)=[D(n-7)+D(n-3)+D(n-2)+D(n-1)] mod 2
Voltage and Current Controlled Elements
HSPICE or HSPICE RF provides two voltage-controlled and two currentcontrolled elements, known as E, G, H, and F Elements. You can use these
controlled elements to model:
156
■
MOS transistors
■
bipolar transistors
■
tunnel diodes
■
SCRs
■
analog functions, such as:
•
operational amplifiers
•
summers
•
comparators
•
voltage-controlled oscillators
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
•
modulators
•
switched capacitor circuits
Depending on whether you used the polynomial or piecewise linear functions,
the controlled elements can be:
■
Linear functions of controlling-node voltages.
■
Non-linear functions of controlling-node voltages.
■
Linear functions of branch currents.
■
Non-linear functions of branch currents.
The functions of the E, F, G, and H controlled elements are different.
■
■
■
The E element can be:
•
A voltage-controlled voltage source
•
A behavioral voltage source
•
An ideal op-amp.
•
An ideal transformer.
•
An ideal delay element.
•
A piecewise linear, voltage-controlled, multi-input AND, NAND, OR, or
NOR gate.
The F element can be:
•
A current-controlled current source.
•
An ideal delay element.
•
A piecewise linear, current-controlled, multi-input AND, NAND, OR, or
NOR gate.
The G element can be:
•
A voltage-controlled current source.
•
A behavioral current source.
•
A voltage-controlled resistor.
•
A piecewise linear, voltage-controlled capacitor.
•
An ideal delay element.
•
A piecewise linear, multi-input AND, NAND, OR, or NOR gate.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
157
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
■
The H element can be:
•
A current-controlled voltage source.
•
An ideal delay element.
•
A piecewise linear, current-controlled, multi-input AND, NAND, OR, or
NOR gate.
The next section describes polynomial and piecewise linear functions. Later
sections describe element statements for linear or nonlinear functions. For
detailed PWL examples, see section “PWL/DATA/VEC Converter” in the
HSPICE Applications Manual.
Polynomial Functions
You can use the controlled element statement to define the controlled output
variable (current, resistance, or voltage), as a polynomial function of one or
more voltages or branch currents. You can select three polynomial equations,
using the POLY(NDIM) parameter in the E, F, G, or H element statement.
Value
Description
POLY(1)
One-dimensional equation (function of one controlling variable).
POLY(2)
Two-dimensional equation (function of two controlling variables).
POLY(3)
Three-dimensional equation (function of three controlling variables).
Each polynomial equation includes polynomial coefficient parameters (P0, P1
… Pn), which you can set to explicitly define the equation.
One-Dimensional Function
If the function is one-dimensional (a function of one branch current or node
voltage), the following expression determines the FV function value:
FV = P0 + ( P1 ⋅ FA ) + ( P2 ⋅ FA 2 ) + ( P3 ⋅ FA 3 ) + ( P4 ⋅ FA 4 ) + ( P5 ⋅ FA 5 ) + …
158
Parameter
Description
FV
Controlled voltage or current, from the controlled source.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
P0. . .PN
Coefficients of a polynomial equation.
FA
Controlling branch current, or nodal voltage.
Note:
If you specify one coefficient in a one-dimensional polynomial, HSPICE or
HSPICE RF assumes that the coefficient is P1 (P0=0.0). Use this as input
for linear controlled sources.
The following controlled source statement is a one-dimensional function. This
voltage-controlled voltage source connects to nodes 5 and 0.
E1 5 0 POLY(1) 3 2 1 2.5
In the above source statement, the single-dimension polynomial function
parameter, POLY(1), informs HSPICE or HSPICE RF that E1 is a function of
the difference of one nodal voltage pair. In this example, the voltage difference
is between nodes 3 and 2, so FA=V(3,2).
The dependent source statement then specifies that P0=1 and P1=2.5. From
the one-dimensional polynomial equation above, the defining equation for
V(5,0) is:
V ( 5, 0 ) = 1 + 2.5 ⋅ V (3,2)
You can also express V(5,0) as E1:
E1 = 1 + 2.5 ⋅ V (3,2)
Two-Dimensional Function
If the function is two-dimensional (that is, a function of two node voltages or two
branch currents), the following expression determines FV:
2
2
FV = P0 + ( P1 ⋅ FA ) + ( P2 ⋅ FB ) + ( P3 ⋅ FA ) + ( P4 ⋅ FA ⋅ FB ) + ( P5 ⋅ FB )
3
2
2
3
+ ( P6 ⋅ FA ) + ( P7 ⋅ FA ⋅ FB ) + ( P8 ⋅ FA ⋅ FB ) + ( P9 ⋅ FB ) + ...
For a two-dimensional polynomial, the controlled source is a function of two
nodal voltages or currents. To specify a two-dimensional polynomial, set
POLY(2) in the controlled source statement.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
159
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
For example, generate a voltage-controlled source that specifies the controlled
voltage, V(1,0), as:
V ( 1, 0 ) = 3 ⋅ V (3,2) + 4 ⋅ V (7,6) 2
or
E1 = 3 ⋅ V (3,2) + 4 ⋅ V (7,6) 2
To implement this function, use this controlled-source element statement:
E1 1 0 POLY(2) 3 2 7 6 0 3 0 0 0 4
This example specifies a controlled voltage source, which connects between
nodes 1 and 0. Two differential voltages control this voltage source:
■
Voltage difference between nodes 3 and 2.
■
Voltage difference between nodes 7 and 6.
That is, FA=V(3,2), and FB=V(7,6). The polynomial coefficients are:
■
P0=0
■
P1=3
■
P2=0
■
P3=0
■
P4=0
■
P5=4
Three-Dimensional Function
For a three-dimensional polynomial function, with FA, FB, and FC as its
arguments, the following expression determines the FV function value:
FV = P0 + ( P1 ⋅ FA ) + ( P2 ⋅ FB ) + ( P3 ⋅ FC ) + ( P4 ⋅ FA 2 )
+ ( P5 ⋅ FA ⋅ FB ) + ( P6 ⋅ FA ⋅ FC ) + ( P7 ⋅ FB 2 ) + ( P8 ⋅ FB ⋅ FC )
+ ( P9 ⋅ FC 2 ) + ( P10 ⋅ FA 3 ) + ( P11 ⋅ FA 2 ⋅ FB ) + ( P12 ⋅ FA 2 ⋅ FC )
+ ( P13 ⋅ FA ⋅ FB 2 ) + ( P14 ⋅ FA ⋅ FB ⋅ FC ) + ( P15 ⋅ FA ⋅ FC 2 )
+ ( P16 ⋅ FB 3 ) + ( P17 ⋅ FB 2 ⋅ FC ) + ( P18 ⋅ FB ⋅ FC 2 )
+ ( P19 ⋅ FC 3 ) + ( P20 ⋅ FA 4 ) + …
160
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
For example, generate a voltage-controlled source that specifies the voltage
as:
V ( 1, 0 ) = 3 ⋅ V (3,2) + 4 ⋅ V (7,6) 2 + 5 ⋅ V (9,8) 3
or
E1 = 3 ⋅ V (3,2) + 4 ⋅ V (7,6) 2 + 5 ⋅ V (9,8) 3
The resulting three-dimensional polynomial equation is:
FA = V (3,2)
FB = V (7,6)
FC = V (9,8)
P1 = 3
P7 = 4
P19 = 5
Substitute these values into the voltage controlled voltage source statement:
E1 1 0 POLY(3) 3 2 7 6 9 8 0 3 0 0 0 0 0 4 0 0 0 0 0 0
+ 0 0 0 0 0 5
The preceding example specifies a controlled voltage source, which connects
between nodes 1 and 0. Three differential voltages control this voltage source:
■
Voltage difference between nodes 3 and 2.
■
Voltage difference between nodes 7 and 6.
■
Voltage difference between nodes 9 and 8.
That is:
■
FA=V(3,2)
■
FB=V(7,6)
■
FC=V(9,8)
The statement defines the polynomial coefficients as:
■
P1=3
■
P7=4
■
P19=5
■
Other coefficients are zero.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
161
Chapter 5: Sources and Stimuli
Voltage and Current Controlled Elements
Piecewise Linear Function
You can use the one-dimensional piecewise linear (PWL) function to model
special element characteristics, such as those of:
■
tunnel diodes
■
silicon-controlled rectifiers
■
diode breakdown regions
To describe the piecewise linear function, specify measured data points.
Although data points describe the device characteristic, HSPICE or HSPICE
RF automatically smooths the corners, to ensure derivative continuity. This, in
turn, results in better convergence.
The DELTA parameter controls the curvature of the characteristic at the
corners. The smaller the DELTA, the sharper the corners are. The maximum
DELTA is limited to half of the smallest breakpoint distance. If the breakpoints
are sufficiently separated, specify the DELTA to a proper value.
■
You can specify up to 100 point pairs.
■
You must specify at least two point pairs (each point consists of an x and a
y coefficient).
To model bidirectional switch or transfer gates, G elements use the NPWL and
PPWL functions, which behave the same way as NMOS and PMOS transistors.
You can also use the piecewise linear function to model multi-input AND,
NAND,OR, and NOR gates. In this usage, only one input determines the state
of the output.
162
■
In AND and NAND gates, the input with the smallest value determines the
corresponding output of the gates.
■
In OR and NOR gates, the input with the largest value determines the
corresponding output of the gates.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Power Sources
Power Sources
This section describes independent sources and controlled sources.
Independent Sources
A power source is a special kind of voltage or current source, which supplies
the network with a pre-defined power that varies by time or frequency. The
source produces a specific input impedance.
To apply a power source to a network, you can use either:
■
A Norton-equivalent circuit (if you specify this circuit and a current source)—
the I (current source) element, or
■
A Thevenin-equivalent circuit (if you specify this circuit and a voltage
source)—the V (voltage source) element.
As with other independent sources, simulation assumes that positive current
flows from the positive node, through the source, to the negative node. A power
source is a time-variant or frequency-dependent utility source; therefore, the
value/phase can be a function of either time or frequency.
A power source is a sub-class of the independent voltage/current source, with
some additional keywords or parameters:
■
You can use I and V elements in DC, AC, and transient analysis.
The I and V elements can be data-driven.
Supported formats include:
■
PULSE, a trapezoidal pulse function.
■
PWL, a piecewise linear function, with repeat function.
■
PL, a piecewise linear function. PWL and PL are the same piecewise linear
function, except PL uses the v1 t1 pair instead of the t1 v1 pair.
■
SIN, a damped sinusoidal function.
■
EXP, an exponential function.
■
SFFM, a single-frequency FM function.
AM, an amplitude-modulation function.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
163
Chapter 5: Sources and Stimuli
Power Sources
Syntax
If you use the power keyword in the netlist, then simulation recognizes a
current/voltage source as a power source:
Vxxx node+ node- power=<powerVal <powerFun>> imp=value1
+ imp_ac=value2,value3 powerFun=<FREQ <TIME>>(...)
Ixxx node+ node- power=<powerVal <powerFun>> imp=value1
+ imp_ac=value2,value3 powerFun=<FREQ <TIME>>(...)
Parameter
Description
powerVal
A constant power source supplies the available power. If you specify
POWER_DB, then the value is in decibels; otherwise, it is in
Watts*POWER_SCAL, where POWER_SCAL is a scaling factor that
you specify in a SCALE option (default=1).
powerFun
This function name indicates the time-variant or frequency-variant
power source. In this equation, powerFun defines the functional
dependence on time or frequency.
■
■
If the function name for powerFun is FREQ, then it is a frequency
power source: FREQ(freq1, val1, freq2, val2,...)
If the function name for powerFun is TIME, then it is a piece-wise
time variant function: TIME(t1, val1, t2, val2...)
imp=
DC impedance value.
imp_ac=
Magnitude and phase offset (in degrees) of AC impedance.
Example 1
V11 10 20 power=5 imp=5K
This example applies a 5-decibel/unit power source to node 10 and node 20, in
a Thevenin-equivalent manner. The impedance of this power source is 5k
Ohms.
Example 2
Iname 1 0 power=20 imp=9MEG
This example applies a 20-decibel/unit power source to node 1 and to ground,
in a Norton-equivalent manner. The source impedance is 9 mega-ohms.
164
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Example 3
V5 6 0 power=FREQ(10HZ, 2, 10KHZ, 0.01) imp=2MEG imp_ac=(100K, 60)
V5 6 0 power=func1 imp=2MEG imp_ac=(100K, 60DEC)
+ func1=FREQ(10HZ, 2, 10KHZ, 0.01)
In the two preceding examples, a power source operates at two different
frequencies, with two different values:
■
At 10 Hz, the power value is 2 decibel/unit.
■
At 10 kHz, the power value is 0.01 decibel/unit.
Also in these examples:
■
The DC impedance is 2 mega-ohms.
■
The AC impedance is 100 kilo-ohms.
■
The phase offset is 60 degrees.
Outputs
None.
Controlled Sources
In addition to independent power sources, you can also create four types of
controlled sources:
■
Voltage-controlled voltage source (VCVS), or E element
■
Current-controlled current source (CCCS), or F element
■
Voltage-controlled current source (VCCS), or G element
■
Current-controlled voltage source (CCVS), or H element
Voltage-dependent Voltage Sources — E Elements
This section explains E Element syntax statements, and defines their
parameters. See also “Using G and E Elements” in the HSPICE Applications
Manual.
■
LEVEL=1 is an OpAmp.
■
LEVEL=2 is a Transformer.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
165
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Voltage-Controlled Voltage Source (VCVS)
Linear
Exxx n+ n- <VCVS> in+ in- gain <MAX=val> <MIN=val>
+ <SCALE=val> <TC1=val> <TC2=val><ABS=1> <IC=val>
For a description of these parameters, see E Element Parameters on
page 173.
Polynomial (POLY)
Exxx n+ n- <VCVS> POLY(NDIM) in1+ in1- ...
+ inndim+ inndim-<TC1=val> <TC2=val> <SCALE=val>
+ <MAX=val> <MIN=val> <ABS=1> p0 <p1…> <IC=val>
In this syntax, dim (dimensions) ≤ 3. For a description of these parameters, see
E Element Parameters on page 173.
Piecewise Linear (PWL)
Exxx n+ n- <VCVS> PWL(1) in+ in- <DELTA=val>
+ <SCALE=val> <TC1=val> <TC2=val> x1,y1 x2,y2
+ x100,y100 <IC=val>
...
For a description of these parameters, see E Element Parameters on
page 173.
Multi-Input Gates
Exxx n+ n- <VCVS> gatetype(k) in1+ in1- ... inj+ inj+ <DELTA=val> <TC1=val> <TC2=val> <SCALE=val>
+ x1,y1 ...
x100,y100 <IC=val>
In this syntax, gatetype(k) can be AND, NAND, OR, or NOR gates. For a
description of these parameters, see E Element Parameters on page 173.
Delay Element
Exxx n+ n- <VCVS> DELAY in+ in- TD=val <SCALE=val>
+ <TC1=val> <TC2=val> <NPDELAY=val>
For a description of these parameters, see E Element Parameters on
page 173.
166
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Laplace Transform
Voltage Gain H(s):
Exxx n+ n- LAPLACE in+ in- k0, k1, ..., kn / d0, d1, ..., dm
+ <SCALE=val> <TC1=val> <TC2=val>
For a description of these parameters, see E Element Parameters on
page 173.
Transconductance H(s):
Gxxx n+ n- LAPLACE in+ in- k0, k1, ..., kn / d0, d1, ..., dm
+ <SCALE=val> <TC1=val> <TC2=val> <M=val>
H(s) is a rational function, in the following form:
k0 + k1 s + … + kn s n
H ( s ) = -------------------------------------------------d0 + d1 s + … + dm s m
You can use parameters to define the values of all coefficients (k0, k1, ..., d0,
d1, ...).
For a description of the G Element parameters, see G Element Parameters on
page 189.
Example
Glowpass 0 out LAPLACE in 0
1.0 / 1.0 2.0 2.0 1.0
Ehipass out 0 LAPLACE in 0 0.0,0.0,0.0,1.0 / 1.0,2.0,2.0,1.0
The Glowpass element statement describes a third-order low-pass filter, with
the transfer function:
1
H ( s ) = ---------------------------------------1 + 2s + 2s 2 + s 3
The Ehipass element statement describes a third-order high-pass filter, with
the transfer function:
s3
H ( s ) = ---------------------------------------1 + 2s + 2s 2 + s 3
HSPICE® Simulation and Analysis User Guide
Y-2006.03
167
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Pole-Zero Function
Voltage Gain H(s):
Exxx n+ n- POLE in+ in- a az1, fz1, ..., azn, fzn / b,
+ ap1, fp1, ..., apm, fpm <SCALE=val> <TC1=val>
+ <TC2=val>
For a description of these parameters, see E Element Parameters on
page 173.
Transconductance H(s):
Gxxx n+ n- POLE in+ in- a az1, fz1, ..., azn, fzn / b,
+ ap1, fp1, ..., apm, fpm <SCALE=val> <TC1=val>
+ <TC2=val> <M=val>
The following equation defines H(s) in terms of poles and zeros:
a ⋅ ( s + α z1 – j2πf z1 )… ( s + α zn – j2πf zn ) ( s + α zn + j2πf zn )
H ( s ) = -----------------------------------------------------------------------------------------------------------------------------------------------------b ⋅ ( s + α p1 – j2πf p1 )… ( s + α pm – j2πf pm ) ( s + α pm + j2πf pm )
The complex poles or zeros are in conjugate pairs. The element description
specifies only one of them, and the program includes the conjugate. You can
use parameters to specify the a, b, α, and f values.
For a description of the G Element parameters, see G Element Parameters on
page 189.
Example
Ghigh_pass 0 out POLE in 0 1.0 0.0,0.0 / 1.0 0.001,0.0
Elow_pass out 0 POLE in 0 1.0 / 1.0, 1.0,0.0 0.5,0.1379
The Ghigh_pass statement describes a high-pass filter, with the transfer
function:
1.0 ⋅ ( s + 0.0 + j ⋅ 0.0 ) H ( s ) = ---------------------------------------------------------1.0 ⋅ ( s + 0.001 + j ⋅ 0.0 )
The Elow_pass statement describes a low-pass filter, with the transfer
function:
1.0
H ( s ) = --------------------------------------------------------------------------------------------------------------------------------------------------1.0 ⋅ ( s + 1 ) ( s + 0.5 + j2π ⋅ 0.1379 ) ( s + 0.5 – ( j2π ⋅ 0.1379 ) )
168
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Frequency Response Table
Voltage Gain H(s):
Exxx n+ n- FREQ in+ in- f1, a1, f1, ..., fi, ai, f1
+ <DELF=val> <MAXF=val> <SCALE=val> <TC1=val>
+ <TC2=val> <LEVEL=val> <ACCURACY=val>
For a description of these parameters, see E Element Parameters on page 173
Transconductance H(s):
Gxxx n+ n- FREQ in+ in- f1, a1, f1, ..., fi, ai, f1
+ <DELF=val> <MAXF=val> <SCALE=val> <TC1=val>
+ <TC2=val> <M=val> <LEVEL=val> <ACCURACY=val>
Where,
■
Each fi is a frequency point, in hertz.
■
ai is the magnitude, in dB.
■
f1 is the phase, in degrees.
At each frequency, HSPICE or HSPICE RF uses interpolation to calculate the
network response, magnitude, and phase. HSPICE or HSPICE RF interpolates
the magnitude (in dB) logarithmically, as a function of frequency. It also
interpolates the phase (in degrees) linearly, as a function of frequency.
ai – ak
H ( j2πf ) = ⎛⎝ -----------------------------⎞⎠ ( log f – log f i ) + a i
log f i – log f k
φi – φk
∠H ( j2πf ) = ⎛ ---------------⎞ ( f – f i ) + φ i
⎝ fi – fk ⎠
For a description of the G Element parameters, see G Element Parameters on
page 189.
Example
Eftable output
+ 1.0k
-3.97m
+ 2.0k
-2.00m
+ 3.0k
17.80m
+ ...... ...
+ 10.0k -53.20
0 FREQ input
293.7
211.0
82.45
0
-1125.5
HSPICE® Simulation and Analysis User Guide
Y-2006.03
169
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
■
The first column is frequency, in hertz.
■
The second column is magnitude, in dB.
■
The third column is phase, in degrees.
Set the LEVEL to 1 for a high-pass filter.
Set the last frequency point to the highest frequency response value that is a
real number, with zero phase.
You can use parameters to set the frequency, magnitude, and phase, in the
table.
Foster Pole-Residue Form
Gain E(s) form
Exxx n+ n+ (Re{A1},
+ (Re{A2},
+ (Re{A3},
+ ...
FOSTER in+ in- k0
Im{A1})/ (Re{p1},
Im{A2})/ (Re{p2},
Im{A3})/ (Re{p3},
k1
Im{p1})
Im{p2})
Im{p3})
For a description of these parameters, see E Element Parameters on
page 173.
Tranconductance G(s) form
Gxxx n+ n+ (Re{A1},
+ (Re{A2},
+ (Re{A3},
+ ...
FOSTER in+ in- k0
Im{A1})/ (Re{p1},
Im{A2})/ (Re{p2},
Im{A3})/ (Re{p3},
k1
Im{p1})
Im{p2})
Im{p3})
In the above syntax, paranthesis , commas, and slashes are separators—they
have the same meaning as a space. A pole-residue pair is represented by four
numbers (real and imaginary part of the residue, then real and imaginary part
of the pole).
You must make sure that Re[pi]<0; otherwise, the simulations will certainly
diverge. Also, it is a good idea to assure passivity of the model (for an N-port
admittance matrix Y, Re{Y} should be positive-definite), or the simulation is
likely to diverge).
For a description of the G Element parameters, see G Element Parameters on
page 189.
170
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Sti-0 TwS
HSPICE® Simulation and Analysis User Guide
Y-2006.03
171
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
+ freq1 noise1
+ freq2 noise2
+ ...
.enddata
The data form defines a basic frequency-noise table. The .DATA statement
contains two parameters: frequency and noise to specify the noise value at
each frequency point. The unit for frequency is hertz, and the unit for noise is
V2/Hz.
Ideal Op-Amp
Exxx n+ n- OPAMP in+ inYou can also substitute LEVEL=1 in place of OPAMP:
Exxx n+ n- in+ in- level=1
For a description of these parameters, see E Element Parameters.
Ideal Transformer
Exxx n+ n- TRANSFORMER in+ in- k
You can also substitute LEVEL=2 in place of TRANSFORMER:
Exxx n+ n- in+ in- level=2 k
For a description of these parameters, see E Element Parameters.
172
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Figure 23
Equivalent VCVS and Ideal Transformer HSPICE Models
VCVS (op-amp) with Gain = g
+
V2
V1
Equivalent HSPICE model
<=>
+
-
V1
V2
V2=g*V2
Ideal transformer with ratio K
I1
V1
k:1
..
Equivalent HSPICE model
I2
I1
I2
V2
<=>
V1
I1=k*I2
+
-
V2
V1=k*V2
E Element Parameters
The E element parameters described in the following list.
Parameter
Description
ABS
Output is an absolute value, if ABS=1.
DELAY
Keyword for the delay element. Same as for the voltage-controlled
voltage source, except it has an associated propagation delay, TD.
This element adjusts propagation delay in macro (subcircuit)
modeling.
DELAY is a reserved word; do not use it as a node name.
DELTA
Controls the curvature of the piecewise linear corners. This
parameter defaults to one-fourth of the smallest distance between
breakpoints. The maximum is one-half of the smallest distance
between breakpoints.
Exxx
Voltage-controlled element name. Must begin with E, followed by
up to 1023 alphanumeric characters.
gain
Voltage gain.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
173
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Parameter
Description
gatetype(k)
Can be AND, NAND, OR, or NOR. k represents the number of
inputs of the gate. x and y represent the piecewise linear variation
of output, as a function of input. In multi-input gates, only one input
determines the state of the output.
IC
Initial condition: initial estimate of controlling voltage value(s). If
you do not specify IC, default=0.0.
in +/-
Positive or negative controlling nodes. Specify one pair for each
dimension.
k
Ideal transformer turn ratio: V(in+,in-) = k ⋅ V(n+,n-) or,
number of gates input.
MAX
Maximum output voltage value. The default is undefined, and sets
no maximum value.
MIN
Minimum output voltage value. The default is undefined, and sets
no minimum value.
n+/-
Positive or negative node of a controlled element.
NDIM
Number of polynomial dimensions. If you do not set POLY(NDIM),
HSPICE or HSPICE RF assumes a one-dimensional polynomial.
NDIM must be a positive number.
NPDELAY
Sets the number of data points to use in delay simulations. The
default value is the larger of either 10, or the smaller of TD/tstep
and tstop/tstep. That is,
min 〈 TD, tstop〉
NPDELAY default = max ---------------------------------------, 10
tstep
The .TRAN statement specifies tstep and tstop values.
OPAMP
or Level=1
174
The keyword for an ideal op-amp element. OPAMP is a HSPICE
reserved word; do not use it as a node name.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Parameter
Description
P0, P1 …
The polynomial coefficients.
If you specify one coefficient, HSPICE or HSPICE RF assumes
that it is P1 (P0=0.0), and that the element is linear.
If you specify more than one polynomial coefficient, the element is
nonlinear, and P0, P1, P2 ... represent them (see Polynomial
Functions on page 158).
POLY
Keyword for the polynomial function. If you do not specify
POLY(ndim), HSPICE assumes a one-dimensional polynomial.
Ndim must be a positive number.
PWL
Keyword for the piecewise linear function.
SCALE
Multiplier for the element value.
TC1,TC2
First-order and second-order temperature coefficients.
Temperature changes update the SCALE:
SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ Δt + TC2 ⋅ Δt 2 )
TD
Keyword for the time (propagation) delay.
TRANSFORMER
or LEVEL=2
Keyword for an ideal transformer. TRANSFORMER is a reserved
word; do not use it as a node name.
VCVS
Keyword for a voltage-controlled voltage source. VCVS is a
reserved word; do not use it as a node name.
x1,...
Controlling voltage across the in+ and in- nodes. The x values
must be in increasing order.
y1,...
Corresponding element values of x.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
175
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
E Element Examples
Ideal OpAmp
You can use the voltage-controlled voltage source to build a voltage amplifier,
with supply limits.
■
The output voltage across nodes 2,3 is v(14,1) * 2.
■
The value of the voltage gain parameter is 2.
■
The MAX parameter sets a maximum E1 voltage of 5 V.
■
The MIN parameter sets a minimum E1 voltage output of -5 V.
Example
If V(14,1)=-4V, then HSPICE or HSPICE RF sets E1 to -5V, and not -8V as the
equation suggests.
Eopamp 2 3 14 1 MAX=+5 MIN=-5 2.0
To specify a value for polynomial coefficient parameters, use the following
format:
.PARAM CU=2.0
E1 2 3 14 1 MAX=+5 MIN=-5 CU
Voltage Summer
An ideal voltage summer specifies the source voltage, as a function of three
controlling voltage(s):
■
V(13,0)
■
V(15,0)
■
V(17,0)
To describe a voltage source, the voltage summer uses this value:
V (13,0) + V (15,0) + V (17,0)
This example represents an ideal voltage summer. It initializes the three
controlling voltages for a DC operating point analysis, to 1.5, 2.0, and 17.25 V.
EX 17 0 POLY(3) 13 0 15 0 17 0 0 1 1 1 IC=1.5,2.0,17.25
176
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Polynomial Function
A voltage-controlled source can also output a non-linear function, using a onedimensional polynomial. This example does not specify the POLY parameter,
so HSPICE or HSPICE RF assumes it is a one-dimensional polynomial—that
is, a function of one controlling voltage. The equation corresponds to the
element syntax. Behavioral equations replace this older method.
V (3,4)=10.5 + 2.1 *V(21,17) + 1.75 *V(21,17)2”
E2 3 4 POLY 21 17 10.5 2.1 1.75
E2 3 4 VOLT=“10.5 + 2.1 *V(21,17) + 1.75 *V(21,17)2”
E2 3 4 POLY 21 17 10.5 2.1 1.75
Zero-Delay Inverter Gate
Use a piecewise linear transfer function to build a simple inverter, with no delay.
Einv out 0 PWL(1) in 0 .7v,5v 1v,0v
Ideal Transformer
If the turn ratio is 10 to 1, the voltage relationship is V(out)=V(in)/10.
Etrans out 0 TRANSFORMER in 0 10
You can also substitute LEVEL=2 in place of TRANSFORMER:
Etrans out 0 in 0 level=2 10
Voltage-Controlled Oscillator (VCO)
The VOL keyword defines a single-ended input, which controls output of a VCO.
Example 1
In this example, the voltage at the control node controls the frequency of the
sinusoidal output voltage at the out node. v0 is the DC offset voltage, and gain
is the amplitude. The output is a sinusoidal voltage, whose frequency is
specified in freq · control.
Evco out 0 VOL=’v0+gain*SIN(6.28 freq*v(control)*TIME)’
Note:
This equation is valid only for a steady-state VCO (fixed voltage). If you
sweep the control voltage, this equation does not apply.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
177
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Example 2
In this example, a Verilog-A module is used to control VCO output by tracking
phase to ensure continuity.
`include "disciplines.vams"
module vco(vin, vout);
inout vin, vout;
electrical vin, vout;
parameter real amp = 1.0;
parameter real offset = 1.0;
parameter real center_freq = 1G;
parameter real vco_gain = 1G;
real phase;
analog begin
phase = idt(center_freq + vco_gain*V(vin), 0.0);
V(vout) <+ offset+amp*sin(6.2831853*phase);
end
endmodule
Example 3
This example is a controlled-source equivalent of the Verilog-A module shown
in the previous example. Like the previous example, it establishes a continuous
phase and therefore, a continuous output voltage.
.subckt vco in out amp=1 offset=1 center_freq=1 vco_gain=1
.ic v(phase)=0
cphase phase 0 1e-10
g1 0 phase cur='1e-10*(center_freq+vco_gain*v(in))'
eout out 0 vol='offset+amp*sin(6.2831853*v(phase))'
.ends
Example 4
In this example, controlled-sources are used to control VCO output.
.param pi=3.1415926
.param twopi='2*pi'
.subckt vco in inb out outb f0=100k kf=50k out_off=0.0 out_amp=1.0
gs 0 s poly(2) c 0 in inb 0 'twopi*1e-9*f0' 0 0 'twopi*1e-9*kf'
gc c 0 poly(2) s 0 in inb 0 'twopi*1e-9*f0' 0 0 'twopi*1e-9*kf'
cs s 0 1e-9 ic=0
cc c 0 1e-9 ic=1
eout out 0 vol='out_off+(out_amp*v(s))'
eoutb outb 0 vol='out_off+(out_amp*v(c))'
.ic v(c)=1 v(s)=0
.ends
178
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-dependent Voltage Sources — E Elements
Using the E Element for AC Analysis
The following equation describes an E element:
E1 ee 0 vol=f(v(1), v(2))
In an AC analysis, voltage is computed as follows:
v(ee)=A * delta_v1 + B * delta_v2
Where,
■
A is the derivative of f(v(1), v(2)) to v(1) at the operating point
■
B is the derivative of f(v(1), v(2)) to v(2) at the operating point
■
delta_v1 is the AC voltage variation of v(1)
■
delta_v2 is the AC voltage variation of v(2)
Example
This example is based on demonstration netlist eelm.sp, which is available in
directory $<installdir>/demo/hspice/sources:
*****************************************************
****** E element for AC analysis
.option post
.op
*CASE1-Mixed and zero time unit has zero value(tran)
v_n1 n1 gnd dc=6.0 pwl 0.0 6.0 1.0n 6.0 ac 5.0
v_n2 n2 gnd dc=4.0 pwl 0.0 4.0 1.0n 6.0 ac 2.0
e1 n3 gnd vol='v(n1)+v(n2)'
e2 n4 gnd vol='v(n1)*v(n2)'
r1 n1 gnd 1
r2 n2 gnd 1
r3 n3 gnd 1
r4 n4 gnd 1
.tran 10p 3n
.ac dec 1 1 100meg
.print ac v(n?)
.end
*****************************************************
The AC voltage of node n3 is:
v(n3)=1.0 *v(n1)(ac)
= 1.0 * 5.0
+
= 7.0 (v)
+ 1.0 * v(n2)(ac)
1.0 * 2.0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
179
Chapter 5: Sources and Stimuli
Current-Dependent Current Sources — F Elements
The AC voltage of node n4 is:
v(n4)=v(n2)(op) * v(n1)(ac) + v(n1)(op) * v(n2)(ac)
= 4.0
*
5.0 + 6.0
* 2.0
= 32.0 (v)
Current-Dependent Current Sources — F Elements
This section explains the F element syntax and parameters.
Current-Controlled Current Source (CCCS) Syntax
Linear
Fxxx n+ n- <CCCS> vn1 gain <MAX=val> <MIN=val> <SCALE=val>
+ <TC1=val> <TC2=val> <M=val> <ABS=1> <IC=val>
Polynomial (POLY)
Fxxx n+ n- <CCCS> POLY(ndim) vn1 <... vnndim> <MAX=val>
+ <MIN=val> <TC1=val> <TC2=val> <SCALE=val> <M=val>
+ <ABS=1> p0 <p1…> <IC=val>
In this syntax, dim (dimensions) ≤ 3.
Piecewise Linear (PWL)
Fxxx n+ n- <CCCS> PWL(1) vn1 <DELTA=val> <SCALE=val>
+ <TC1=val> <TC2=val> <M=val> x1,y1 ... x100,y100 <IC=val>
Multi-Input Gates
Fxxx n+ n- <CCCS> gatetype(k) vn1, ... vnk <DELTA=val>
+ <SCALE=val> <TC1=val> <TC2=val> <M=val> <ABS=1>
+ x1,y1 ...
x100,y100 <IC=val>
In this syntax, gatetype(k) can be AND, NAND, OR, or NOR gates.
180
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Current-Dependent Current Sources — F Elements
Delay Element
Note:
G elements with algebraics make F elements obsolete. You can still use F
elements for backward-compatibility with existing designs.
Fxxx n+ n- <CCCS> DELAY vn1 TD=val <SCALE=val>
+ <TC1=val><TC2=val> NPDELAY=val
F Element Parameters
The F Element parameters are described in the following list.
Parameter
Description
ABS
Output is an absolute value, if ABS=1.
CCCS
Keyword for current-controlled current source. CCCS is a HSPICE
reserved keyword; do not use it as a node name.
DELAY
Keyword for the delay element. Same as for a current-controlled current
source, but has an associated propagation delay, TD. Adjusts the
propagation delay in the macro model (subcircuit) process. DELAY is a
reserved word; do not use it as a node name.
DELTA
Controls the curvature of piecewise linear corners. The default is 1/4 of
the smallest distance between breakpoints. The maximum is 1/2 of the
smallest distance between breakpoints.
Fxxx
Element name of the current-controlled current source. Must begin with
F, followed by up to 1023 alphanumeric characters.
gain
Current gain.
gatetype(k)
AND, NAND, OR, or NOR. k is the number of inputs for the gate. x and
y are the piecewise linear variation of the output, as a function of input.
In multi-input gates, only one input determines the output state. Do not
use the above keywords as node names.
IC
Initial condition (estimate) of the controlling current(s), in amps. If you
do not specify IC, the default=0.0.
M
Number of replications of the element, in parallel.
MAX
Maximum output current. Default=undefined; sets no maximum.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
181
Chapter 5: Sources and Stimuli
Current-Dependent Current Sources — F Elements
Parameter
Description
MIN
Minimum output current. Default=undefined; sets no minimum.
n+/-
Connecting nodes for a positive or negative controlled source.
NDIM
Number of polynomial dimensions. If you do not specify POLY(NDIM),
HSPICE or HSPICE RF assumes a one-dimensional polynomial. NDIM
must be a positive number.
NPDELAY
Number of data points to use in delay simulations. The default value is
the larger of either 10, or the smaller of TD/tstep and tstop/tstep. That
min 〈 TD, tstop〉
is, NPDELAY default = max ---------------------------------------, 10
tstep
The .TRAN
statement specifies the tstep and tstop values.
P0, P1 …
The polynomial coefficients.
If you specify one coefficient, HSPICE or HSPICE RF assumes it is P1
(P0=0.0), and the source element is linear.
If you specify more than one polynomial coefficient, then the source is
non-linear, and HSPICE or HSPICE RF assumes that the polynomials
are P0, P1, P2 … See Polynomial Functions on page 158.
POLY
Keyword for the polynomial function. If you do not specify POLY(ndim),
HSPICE assumes that this is a one-dimensional polynomial. Ndim must
be a positive number.
PWL
Keyword for the piecewise linear function.
SCALE
Multiplier for the element value.
TC1,TC2
First-order and second-order temperature coefficients. Temperature
changes update the SCALE:
SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ Δt + TC2 ⋅ Δt 2 )
182
TD
Keyword for the time (propagation) delay.
vn1 …
Names of voltage sources, through which the controlling current flows.
Specify one name for each dimension.
x1,...
Controlling current, through the vn1 source. Specify the x values in
increasing order.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Current-Dependent Current Sources — F Elements
Parameter
Description
y1,...
Corresponding output current values of x.
F Element Examples
Example 1
This example describes a current-controlled current source, connected
between nodes 13 and 5. The current, which controls the value of the
controlled source, flows through the voltage source named VSENS.
F1 13 5 VSENS MAX=+3 MIN=-3 5
Note:
To use a current-controlled current source, you can place a dummy
independent voltage source into the path of the controlling current.
The defining equation is:
I ( F1 ) = 5 ⋅ I ( VSENS )
■
Current gain is 5.
■
Maximum current flow through F1 is 3 A.
■
Minimum current flow is -3 A.
If I(VSENS)=2 A, then this examples sets I(F1) to 3 amps, not 10 amps (as
the equation suggests). You can define a parameter for the polynomial
coefficient(s):
.PARAM VU=5
F1 13 5 VSENS MAX=+3 MIN=-3 VU
Example 2
This example is a current-controlled current source, with the value:
I(F2)=1e-3 + 1.3e-3 ⋅ I(VCC)
Current flows from the positive node, through the source, to the negative node.
The positive controlling-current flows from the positive node, through the
source, to the negative node of vnam (linear), or to the negative node of each
voltage source (nonlinear).
F2 12 10 POLY VCC 1MA 1.3M
HSPICE® Simulation and Analysis User Guide
Y-2006.03
183
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Example 3
This example is a delayed, current-controlled current source.
Fd 1 0 DELAY vin TD=7ns SCALE=5
Example 4
This example is a piecewise-linear, current-controlled current source.
Filim 0 out PWL(1) vsrc -1a,-1a 1a,1a
Voltage-Dependent Current Sources — G Elements
This section explains G element syntax statements, and their parameters.
■
LEVEL=0 is a Voltage-Controlled Current Source (VCCS).
■
LEVEL=1 is a Voltage-Controlled Resistor (VCR).
■
LEVEL=2 is a Voltage-Controlled Capacitor (VCCAP), Negative Piece-Wise
Linear (NPWL).
■
LEVEL=3 is a VCCAP, Positive Piece-Wise Linear (PPWL).
See also “Using G and E Elements” in the HSPICE Applications Manual.
Voltage-Controlled Current Source (VCCS)
Linear
Gxxx n+ n- <VCCS> in+ in- transconductance <MAX=val>
+ <MIN=val> <SCALE=val> <M=val> <TC1=val> <TC2=val>
+ <ABS=1> <IC=val>
For a description of the G Element parameters, see G Element Parameters on
page 189.
Polynomial (POLY)
Gxxx n+ n- <VCCS> POLY(NDIM) in1+ in1- ... <inndim+ inndim->
+ <MAX=val> <MIN=val> <SCALE=val> <M=val> <TC1=val>
+ <TC2=val> <ABS=1> P0<P1…> <IC=vals>
For a description of the G Element parameters, see G Element Parameters on
page 189.
184
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Piecewise Linear (PWL)
Gxxx n+ n- <VCCS> PWL(1) in+ in- <DELTA=val>
+ <SCALE=val> <M=val> <TC1=val> <TC2=val>
+ x1,y1 x2,y2 ... x100,y100 <IC=val> <SMOOTH=val>
Gxxx n+ n- <VCCS> NPWL(1) in+ in- <DELTA=val>
+ <SCALE=val> <M=val> <TC1=val><TC2=val>
+ x1,y1 x2,y2 ... x100,y100 <IC=val> <SMOOTH=val>
Gxxx n+ n- <VCCS> PPWL(1) in+ in- <DELTA=val>
+ <SCALE=val> <M=val> <TC1=val> <TC2=val>
+ x1,y1 x2,y2 ... x100,y100 <IC=val> <SMOOTH=val>
For a description of the G Element parameters, see G Element Parameters on
page 189.
Multi-Input Gate
Gxxx n+ n- <VCCS> gatetype(k) in1+ in1- ...
+ ink+ ink- <DELTA=val> <TC1=val> <TC2=val> <SCALE=val>
+ <M=val> x1,y1 ... x100,y100<IC=val>
In this syntax, gatetype(k) can be AND, NAND, OR, or NOR gates. For a
description of the G Element parameters, see G Element Parameters on
page 189.
Delay Element
Gxxx n+ n- <VCCS> DELAY in+ in- TD=val <SCALE=val>
+ <TC1=val> <TC2=val> NPDELAY=val
For a description of the G Element parameters, see G Element Parameters on
page 189.
Laplace Transform
For details, see Laplace Transform on page 167.
Pole-Zero Function
For details, see Pole-Zero Function on page 168.
Frequency Response Table
For details, see Frequency Response Table on page 169.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
185
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Foster Pole-Residue Form
For details, see Foster Pole-Residue Form on page 170.
Behavioral Current Source (Noise Model)
Expression form
gxxx node1 node2 noise=’noise_expression’
The xxx parameter can be set with a value up to 1024 characters. The node1
and node2 are the positive and negative nodes that connect to the noise
source. The noise expression can contain the bias, frequency, or other
parameters, and involve node voltages and currents through voltage sources.
For a description of the G Element parameters, see G Element Parameters on
page 189.
This syntax creates a simple two-terminal current noise source, whose value is
described in A2/Hz. The output noise generated from this noise source is:
noise_expression*H
H is the transfer function from the terminal pair (node1,node2) to the circuit
output, where the output noise is measured.
You can also implement a behavioral noise source with an E Element. As noise
elements, they are two-terminal elements that represent a noise source
connected between two specified nodes.
gname node1 node2 node3 node4 noise=’expression’
This syntax produces a noise source correlation between the terminal pairs
(node1 node2) and (node3 node4). The resulting output noise is computed
as:
noise_expression*sqrt(H1*H2*)
■
H1 is the transfer function from (node1,node2) to the output.
■
H2 is the transfer function from (node3,node4) to the output.
The noise expression can involve node voltages and currents through voltage
sources.
Data form
Gxxx node1 node2 noise data=dataname
.DATA dataname
+ pname1 pname2
186
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
+ freq1 noise1
+ freq2 noise2
+ ...
.enddata
The data form defines a basic frequency-noise table. The .DATA statement
contains two parameters: frequency and noise to specify the noise value at
each frequency point. The unit for frequency is hertz, and the unit for noise is
A2/Hz.
For a description of the G Element parameters, see G Element Parameters on
page 189.
Example
The following netlist shows a 1000 ohm resistor (g1) using a G element. The
g1noise element, placed in parallel with the g1 resistor, delivers the thermal
noise expected from a resistor. The r1 resistor is included for comparison: The
noise due to r1 should be the same as the noise due to g1noise.
* Resistor implemented using g-element
v1 1 0 1
r1 1 2 1k
g1 1 2 cur='v(1,2)*0.001'
g1noise 1 2
+ noise='4*1.3806266e-23*(TEMPER+273.15)*0.001'
rout 2 0 1meg
.ac lin 1 100 100
.noise v(2) v1 1
.end
Voltage-Controlled Resistor (VCR)
Linear
Gxxx n+ n- VCR in+ in- transfactor <MAX=val> <MIN=val>
+ <SCALE=val> <M=val> <TC1=val> <TC2=val> <IC=val>
For a description of the G Element parameters, see G Element Parameters on
page 189.
Polynomial (POLY)
Gxxx n+ n- VCR POLY(NDIM) in1+ in1- ...
+ <inndim+ inndim-> <MAX=val> <MIN=val><SCALE=val>
+ <M=val> <TC1=val> <TC2=val>
P0 <P1…> <IC=vals>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
187
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
For a description of the G Element parameters, see G Element Parameters on
page 189.
Piecewise Linear (PWL)
Gxxx n+ n- VCR PWL(1) in+ in- <DELTA=val> <SCALE=val>
+ <M=val> <TC1=val> <TC2=val> x1,y1 x2,y2 ... x100,y100
+ <IC=val> <SMOOTH=val>
Gxxx n+ n- VCR NPWL(1) in+ in- <DELTA=val> <SCALE=val>
+ <M=val> <TC1=val> <TC2=val> x1,y1 x2,y2 ... x100,y100
+ <IC=val> <SMOOTH=val>
Gxxx n+ n- VCR PPWL(1) in+ in- <DELTA=val> <SCALE=val>
+ <M=val> <TC1=val> <TC2=val> x1,y1 x2,y2 ... x100,y100
+ <IC=val> <SMOOTH=val>
For a description of the G Element parameters, see G Element Parameters on
page 189.
Multi-Input Gates
Gxxx n+ n- VCR gatetype(k) in1+ in1- ... ink+ ink+ <DELTA=val> <TC1=val> <TC2=val> <SCALE=val> <M=val>
+ x1,y1 ... x100,y100 <IC=val>
For a description of the G Element parameters, see G Element Parameters on
page 189.
Voltage-Controlled Capacitor (VCCAP)
Gxxx n+ n- VCCAP PWL(1) in+ in<DELTA=val>
+ <SCALE=val> <M=val> <TC1=val> <TC2=val>
+ x1,y1 x2,y2 ... x100,y100 <IC=val> <SMOOTH=val>
HSPICE or HSPICE RF uses either LEVEL=2 (NPWL) or LEVEL=3 (PPWL),
based on the relationship of the (n+, n-) and (in+, in-) nodes. For a description
of the G Element parameters, see G Element Parameters on page 189.
Use the NPWL and PPWL functions to interchange the n+ and n- nodes, but use
the same transfer function. The following summarizes this action:
188
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
NPWL Function
For the in- node connected to n+:
■
If v(n+,n-) < 0, then the controlling voltage is v(in+,in-).
■
Otherwise, the controlling voltage is v(in+,n-).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
189
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
190
Parameter
Description
DELAY
Keyword for the delay element. Same as in the voltage-controlled
current source, but has an associated propagation delay, TD.
Adjusts propagation delay in macro (subcircuit) modeling. DELAY
is a keyword; do not use it as a node name.
DELTA
Controls curvature of piecewise linear corners. Defaults to 1/4 of
the smallest distance between breakpoints. Maximum is 1/2 of the
smallest distance between breakpoints.
Gxxx
Name of the voltage-controlled element. Must begin with G,
followed by up to 1023 alphanumeric characters.
gatetype(k)
AND, NAND, OR, or NOR. The k parameter is the number of inputs
of the gate. x and y represent the piecewise linear variation of the
output, as a function of the input. In multi-input gates, only one
input determines the state of the output.
IC
Initial condition. Initial estimate of the value(s) of controlling
voltage(s). If you do not specify IC, the default=0.0.
in +/-
Positive or negative controlling nodes. Specify one pair for each
dimension.
M
Number of replications of the elements in parallel.
MAX
Maximum value of the current or resistance. The default is
undefined, and sets no maximum value.
MIN
Minimum value of the current or resistance. The default is
undefined, and sets no minimum value.
n+/-
Positive or negative node of the controlled element.
NDIM
Number of polynomial dimensions. If you do not specify
POLY(NDIM), HSPICE assumes a one-dimensional polynomial.
NDIM must be a positive number.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Parameter
Description
NPDELAY
Sets the number of data points to use in delay simulations. The
default value is the larger of either 10, or the smaller of TD/tstep
and tstop/tstep. That is,
min 〈 TD, tstop〉
NPDELAY default = max ---------------------------------------, 10
tstep
.
The .TRAN statement specifies the tstep and tstop values.
NPWL
Models symmetrical bidirectional switch/transfer gate, NMOS.
P0, P1 …
The polynomial coefficients.
■
■
If you specify one coefficient, HSPICE or HSPICE RF assumes
that it is P1 (P0=0.0), and the element is linear.
If you specify more than one polynomial coefficient, the element
is non-linear, and the coefficients are P0, P1, P2 ... (see
Polynomial Functions on page 158).
POLY
Keyword for the polynomial dimension function. If you do not
specify POLY(ndim), HSPICE assumes that it is a one-dimensional
polynomial. Ndim must be a positive number.
PWL
Keyword for the piecewise linear function.
PPWL
Models symmetrical bidirectional switch/transfer gate, PMOS.
SCALE
Multiplier for the element value.
SMOOTH
For piecewise-linear, dependent-source elements, SMOOTH
selects the curve-smoothing method.
A curve-smoothing method simulates exact data points that you
provide. You can use this method to make HSPICE or HSPICE RF
simulate specific data points, which correspond to either measured
data or data sheets.
Choices for SMOOTH are 1 or 2:
■
■
Selects the smoothing method used in Hspice versions before
release H93A. Use this method to maintain compatibility with
simulations that you ran, using releases older than H93A.
Selects the smoothing method, which uses data points that you
provide. This is the default for Hspice versions starting with
release H93A.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
191
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Parameter
Description
TC1,TC2
First-order and second-order temperature coefficients.
Temperature changes update the
SCALE:
TD
SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ Δt + TC2 ⋅ Δt 2 ) .
Keyword for the time (propagation) delay.
transconductance Voltage-to-current conversion factor.
transfactor
Voltage-to-resistance conversion factor.
VCCAP
Keyword for voltage-controlled capacitance element. VCCAP is a
reserved HSPICE keyword; do not use it as a node name.
VCCS
Keyword for the voltage-controlled current source. VCCS is a
reserved HSPICE keyword; do not use it as a node name.
VCR
Keyword for the voltage controlled resistor element. VCR is a
reserved HSPICE keyword; do not use it as a node name.
x1,...
Controlling voltage, across the in+ and in- nodes. Specify the
x values in increasing order.
y1,...
Corresponding element values of x.
G Element Examples
Switch
A voltage-controlled resistor represents a basic switch characteristic. The
resistance between nodes 2 and 0 varies linearly, from 10 meg to 1 m ohms,
when voltage across nodes 1 and 0 varies between 0 and 1 volt. The
resistance remains at 10 meg when below the lower voltage limit, and at 1 m
ohms when above the upper voltage limit.
Gswitch 2 0 VCR PWL(1) 1 0 0v,10meg 1v,1m
Switch-Level MOSFET
To model a switch level n-channel MOSFET, use the N-piecewise linear
resistance switch. The resistance value does not change when you switch the d
and s node positions.
192
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Gnmos d s VCR NPWL(1) g s LEVEL=1 0.4v,150g
+ 1v,10meg 2v,50k 3v,4k 5v,2k
Voltage-Controlled Capacitor
The capacitance value across the (out,0) nodes varies linearly (from 1 p to 5 p),
when voltage across the ctrl,0 nodes varies between 2 v and 2.5 v. The
capacitance value remains constant at 1 picofarad when below the lower
voltage limit, and at 5 picofarads when above the upper voltage limit.
Gcap out 0 VCCAP PWL(1) ctrl 0 2v,1p 2.5v,5p
Zero-Delay Gate
To implement a two-input AND gate, use an expression and a piecewise linear
table.
■
The inputs are voltages at the a and b nodes.
■
The output is the current flow from the out to 0 node.
■
HSPICE or HSPICE RF multiplies the current by the SCALE value—which in
this example, is the inverse of the load resistance, connected across the
out,0 nodes.
Gand out 0 AND(2) a 0 b 0 SCALE=’1/rload’ 0v,0a 1v,.5a
+ 4v,4.5a 5v,5a
Delay Element
A delay is a low-pass filter type delay, similar to that of an opamp. In contrast, a
transmission line has an infinite frequency response. A glitch input to a G delay
attenuates in a way that is similar to a buffer circuit. In this example, the output
of the delay element is the current flow, from the out node to the 1 node, with a
value equal to the voltage across the (in, 0) nodes, multiplied by the SCALE
value, and delayed by the TD value.
Gdel out 0 DELAY in 0 TD=5ns SCALE=2 NPDELAY=25
Diode Equation
To model forward-bias diode characteristics, from node 5 to ground, use a
runtime expression. The saturation current is 1e-14 amp, and the thermal
voltage is 0.025 v.
Gdio 5 0 CUR=’1e-14*(EXP(V(5)/0.025)-1.0)’
HSPICE® Simulation and Analysis User Guide
Y-2006.03
193
Chapter 5: Sources and Stimuli
Voltage-Dependent Current Sources — G Elements
Diode Breakdown
You can model the diode breakdown region to a forward region. When voltage
across a diode is above or below the piecewise linear limit values (-2.2v, 2v),
the diode current remains at the corresponding limit values (-1a, 1.2a).
Gdiode 1 0 PWL(1) 1 0 -2.2v,-1a -2v,-1pa .3v,.15pa
+.6v,10ua 1v,1a 2v,1.2a
Triodes
Both of the following voltage-controlled current sources implement a basic
triode.
■
The first example uses the poly(2) operator, to multiply the anode and grid
voltages together, and to scale by .02.
■
The second example uses the explicit behavioral algebraic description.
gt i_anode cathode poly(2) anode,cathode
+ grid,cathode 0 0 0 0 .02
gt i_anode cathode
+ cur=’20m*v(anode,cathode)*v(grid,cathode)’
Behavioral Noise Model
The following netlist shows a 1000 Ohm resistor (g1) implemented using a G
element. The g1noise element, placed in parallel with the g1 resistor, delivers
the thermal noise expected from a resistor. The r1 resistor is included for
comparison: the noise due to r1 should be the same as the noise due to
g1noise.
* Resistor implemented using g-element
v1 1 0 1
r1 1 2 1k
g1 1 2 cur='v(1,2)*0.001'
g1noise 1 2 noise='sqrt(4*1.3806266e-23*(TEMPER+273.15)*0.001)'
rout 2 0 1meg
.ac lin 1 100 100
.noise v(2) v1 1
.end
194
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Current-Dependent Voltage Sources — H Elements
Current-Dependent Voltage Sources — H Elements
This section explains H element syntax statements, and defines their
parameters.
Current-Controlled Voltage Source (CCVS)
Linear
Hxxx n+ n- <CCVS> vn1 transresistance <MAX=val> <MIN=val>
+ <SCALE=val> <TC1=val><TC2=val> <ABS=1> <IC=val>
Polynomial (POLY)
Hxxx n+ n- <CCVS> POLY(NDIM) vn1 <... vnndim>
+ <MAX=val><MIN=val> <TC1=val> <TC2=val> <SCALE=val>
+ <ABS=1> P0 <P1…> <IC=val>
Piecewise Linear (PWL)
Hxxx n+ n- <CCVS> PWL(1) vn1 <DELTA=val> <SCALE=val>
+ <TC1=val> <TC2=val> x1,y1 ...
x100,y100 <IC=val>
Multi-Input Gate
Hxxx n+ n- gatetype(k) vn1, ...vnk <DELTA=val> <SCALE=val>
+ <TC1=val> <TC2=val> x1,y1 ...
x100,y100 <IC=val>
In this syntax, gatetype(k) can be AND, NAND, OR, or NOR gates.
Delay Element
Note:
E elements with algebraics make CCVS elements obsolete. You can still use
CCVS elements for backward-compatibility with existing designs.
Hxxx n+ n- <CCVS> DELAY vn1 TD=val <SCALE=val> <TC1=val>
+ <TC2=val> <NPDELAY=val>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
195
Chapter 5: Sources and Stimuli
Current-Dependent Voltage Sources — H Elements
196
Parameter
Description
ABS
Output is an absolute value, if ABS=1.
CCVS
Keyword for the current-controlled voltage source. CCVS is a
HSPICE reserved keyword; do not use it as a node name.
DELAY
Keyword for the delay element. Same as for a current-controlled
voltage source, but has an associated propagation delay, TD. Use
this element to adjust the propagation delay in the macro
(subcircuit) model process. DELAY is a HSPICE reserved keyword;
do not use it as a node name.
DELTA
Controls curvature of piecewise linear corners. The default is 1/4 of
the smallest distance between breakpoints. Maximum is 1/2 of the
smallest distance between breakpoints.
gatetype(k)
Can be AND, NAND, OR, or NOR. The k value is the number of
inputs of the gate. The x and y terms are the piecewise linear
variation of the output, as a function of the input. In multi-input
gates, one input determines the output state.
Hxxx
Element name of current-controlled voltage source. Must start with
H, followed by up to 1023 alphanumeric characters.
IC
Initial condition (estimate) of the controlling current(s), in amps. If
you do not specify IC, the default=0.0.
MAX
Maximum voltage. Default is undefined; sets no maximum.
MIN
Minimum voltage. Default is undefined; sets no minimum.
n+/-
Connecting nodes for positive or negative controlled source.
NDIM
Number of polynomial dimensions. If you do not specify
POLY(NDIM), HSPICE or HSPICE RF assumes a one-dimensional
polynomial. NDIM must be a positive number.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Current-Dependent Voltage Sources — H Elements
Parameter
Description
NPDELAY
Number of data points to use in delay simulations. The default value
is the larger of either 10, or the smaller of TD/tstep and tstop/tstep.
min 〈 TD, tstop〉
tstep
That is: NPDELAY default = max ---------------------------------------, 10
.
The .TRAN statement specifies the tstep and tstop values.
P0, P1 . . .
Polynomial coefficients.
■
■
If you specify one polynomial coefficient, the source is linear, and
HSPICE or HSPICE RF assumes that the polynomial is P1
(P0=0.0).
If you specify more than one polynomial coefficient, the source
is non-linear. HSPICE assumes the polynomials are P0, P1, P2
… See Polynomial Functions on page 158.
POLY
Keyword for polynomial dimension function. If you do not specify
POLY(ndim), HSPICE assumes a one-dimensional polynomial.
Ndim must be a positive number.
PWL
Keyword for a piecewise linear function.
SCALE
Multiplier for the element value.
TC1,TC2
First-order and second-order temperature coefficients.
Temperature changes update the SCALE:
SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ Δt + TC2 ⋅ Δt 2 )
TD
Keyword for the time (propagation) delay.
transresistance
Current-to-voltage conversion factor.
vn1 …
Names of voltage sources, through which controlling current flows.
You must specify one name for each dimension.
x1,...
Controlling current, through the vn1 source. Specify the x values in
increasing order.
y1,...
Corresponding output voltage values of x.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
197
Chapter 5: Sources and Stimuli
Current-Dependent Voltage Sources — H Elements
Example 1
HX 20 10 VCUR MAX=+10 MIN=-10 1000
The example above selects a linear current-controlled voltage source. The
controlling current flows through the dependent voltage source, called VCUR.
Example 2
The defining equation of the CCVS is:
HX = 1000 ⋅ I ( VCUR )
The defining equation specifies that the voltage output of HX is 1000 times the
value of the current flowing through VCUR.
■
If the equation produces a value of HX greater than +10 V, then the MAX
parameter sets HX to 10 V.
■
If the equation produces a value of HX less than -10 V, then the MIN
parameter sets HX to -10 V.
VCUR is the name of the independent voltage source, through which the
controlling current flows. If the controlling current does not flow through an
independent voltage source, you must insert a dummy independent voltage
source.
Example 3
.PARAM CT=1000
HX 20 10 VCUR MAX=+10 MIN=-10 CT
HXY 13 20 POLY(2) VIN1 VIN2 0 0 0 0 1 IC=0.5, 1.3
The example above describes a dependent voltage source, with the value:
V = I ( VIN1 ) ⋅ I ( VIN2 )
This two-dimensional polynomial equation specifies:
198
■
FA1=VIN1
■
FA2=VIN2
■
P0=0
■
P1=0
■
P2=0
■
P3=0
■
P4=1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
The initial controlling current is .5 mA through VIN1, and 1.3 mA for VIN2.
Positive controlling current flows from the positive node, through the source, to
the negative node of vnam (linear). The (non-linear) polynomial specifies the
source voltage, as a function of the controlling current(s).
Digital and Mixed Mode Stimuli
HSPICE input netlists support two types of digital stimuli:
■
U element digital input files (HSPICE only).
■
Vector input files (HSPICE or HSPICE RF).
This section describes both types.
U Element Digital Input Elements and Models
This section describes the input file format for a U Element. For a description of
the U Element, see the “Modeling Ideal and Lumped Transmission Lines”
chapter in the HSPICE Signal Integrity Guide.
In HSPICE (but not in HSPICE RF), the U Element can reference digital input
and digital output models for mixed-mode simulation. If you run HSPICE in
standalone mode, the state information originates from a digital file. Digital
outputs are handled in a similar fashion. In digital input file mode, the input file
is named <design>.d2a, and the output file is named <design>.a2d.
A2D and D2A functions accept the terminal “\” backslash character as a linecontinuation character, to allow more than 255 characters in a line. Use line
continuation if the first line of a digital file, which contains the signal name list, is
longer than the maximum line length that your text editor accepts.
Do not put a blank first line in a digital D2A file. If the first line of a digital file is
blank, HSPICE issues an error message.
Example
The following example demonstrates how to use the “\” line continuation
character, to format an input file for text editing. The example file contains a
signal list for a 64-bit bus.
...
a00 a01 a02 a03 a04 a05 a06 a07 \
a08 a09 a10 a11 a12 a13 a14 a15 \
... * Continuation of signal names
HSPICE® Simulation and Analysis User Guide
Y-2006.03
199
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
a56 a57 a58 a59 a60 a61 a62 a63 End of signal names
... Remainder of file
General Form
Uxxx interface nlo nhi mname SIGNAME=sname IS=val
Parameter
Description
Uxxx
Digital input element name. Must begin with U, followed by up to 1023
alphanumeric characters.
interface
Interface node in the circuit, to which the digital input attaches.
nlo
Node connected to the low-level reference.
nhi
Node connected to the high-level reference.
mname
Digital input model reference (U model).
SIGNAME
Signal name, as referenced in the digital output file header. Can be a
string of up to eight alphanumeric characters.
IS
Initial state of the input element. Must be a state that the model defines.
Model Syntax
.MODEL mname U LEVEL=5 <parameters...>
Digital input (not supported in HSPICE RF).
Digital-to-Analog Input Model Parameters
Table 12
Names (Alias)
Units
Default
Description
CLO
farad
0
Capacitance, to low-level node.
CHI
farad
0
Capacitance, to high-level node.
S0NAME
200
Digital-to-Analog Parameters
State 0 character abbreviation. A string of up
to four alphanumerical characters.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
Table 12
Digital-to-Analog Parameters (Continued)
Names (Alias)
Units
Default
S0TSW
sec
State 0 switching time.
S0RLO
ohm
State 0 resistance, to low-level node.
S0RHI
ohm
State 0 resistance, to high-level node.
S1NAME
Description
State 1 character abbreviation. A string of up
to four alphanumerical characters.
S1TSW
sec
State 1 switching time.
S1RLO
ohm
State 1 resistance, to low-level node.
S1RHI
ohm
State 1 resistance, to high-level node.
S19NAME
State 19 character abbreviation. A string of
up to four alphanumerical characters.
S19TSW
sec
State 19 switching time.
S19RLO
ohm
State 19 resistance, to low-level node.
S19RHI
ohm
State 19 resistance, to high-level node.
TIMESTEP
sec
Step size for digital input files only.
To define up to 20 different states in the model definition, use the SnNAME,
SnTSW, SnRLO and SnRHI parameters, where n ranges from 0 to 19.
Figure 24 is the circuit representation of the element.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
201
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
Figure 24
Digital-to-Analog Converter Element
RHI
Node to
Hi_ref
source
CHI
CLO
Node to
Low_ref
source
Interface
Node
RLO
Example
The following example shows how to use the U element and model, as a digital
input for a HSPICE netlist (you cannot use the U element in a HSPICE RF
netlist).
This example is based on demonstration netlist uelm.sp, which is available in
directory $<installdir>/demo/hspice/sources:
* EXAMPLE OF U-ELEMENT DIGITAL INPUT
.option post
UC carry-in VLD2A VHD2A D2A SIGNAME=1 IS=0
VLO VLD2A GND DC 0
VHI VHD2A GND DC 1
.MODEL D2A U LEVEL=5 TIMESTEP=1NS,
+ S0NAME=0 S0TSW=1NS S0RLO = 15, S0RHI = 10K,
+ S2NAME=x S2TSW=3NS S2RLO = 1K, S2RHI = 1K
+ S3NAME=z S3TSW=5NS S3RLO = 1MEG,S3RHI = 1MEG
+ S4NAME=1 S4TSW=1NS S4RLO = 10K, S4RHI = 60
.PRINT V(carry-in)
.TRAN 1N 100N
.END
The associated digital input file is:
1
00
09
10
11
20
30
39
40
41
202
1:1
z:1
0:1
z:1
1:1
0:1
x:1
1:1
x:1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
50
60
70
80
0:1
1:1
0:1
1:1
U Element Digital Outputs
Digital output (not supported in HSPICE RF).
Syntax
Uxxx interface reference mname SIGNAME=sname
Parameter
Description
Uxxx
Digital output element name. Must begin with U, followed by up to 1023
alphanumeric characters.
interface
Interface node in the circuit, at which HSPICE measures the digital
output.
reference
Node to use as a reference for the output.
mname
Digital output model reference (U model).
SIGNAME
Signal name, as referenced in the digital output file header. A string of
up to eight alphanumeric characters.
Model Syntax
.MODEL mname U LEVEL=4 <parameters...>
Analog-to-Digital Output Model Parameters
Table 13
Analog-to-Digital Parameters
Name (Alias)
Units
Default
Description
RLOAD
ohm
1/gmin
Output resistance.
CLOAD
farad
0
Output capacitance.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
203
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
Table 13
Analog-to-Digital Parameters (Continued)
Name (Alias)
Units
Default
S0NAME
State 0 character abbreviation. A string of up
to four alphanumerical characters.
S0VLO
volt
State 0 low-level voltage.
S0VHI
volt
State 0 high-level voltage.
S1NAME
State 1 character abbreviation. A string of up
to four alphanumerical characters.
S1VLO
volt
State 1 low-level voltage.
S1VHI
volt
State 1 high-level voltage.
S19NAME
State 19 character abbreviation. A string of
up to four alphanumerical characters.
S19VLO
volt
State 19 low-level voltage.
S19VHI
volt
State 19 high-level voltage.
TIMESTEP
sec
TIMESCALE
204
Description
1E-9
Step size for digital input file.
Scale factor for time.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Digital and Mixed Mode Stimuli
To define up to 20 different states in the model definition, use the SnNAME,
SnVLO and SnVHI parameters, where n ranges from 0 to 19. Figure 25 shows
the circuit representation of the element.
Figure 25
Analog-to-Digital Converter Element
Interface Node
CLOAD
RLOAD
Analog-to-Digital
state conversion by
U model (level=4)
Reference Node
HSPICE® Simulation and Analysis User Guide
Y-2006.03
205
Chapter 5: Sources and Stimuli
Replacing Sources With Digital Inputs
Replacing Sources With Digital Inputs
Figure 26
Digital File Signal Correspondence
V1 carry-in gnd PWL(0NS,lo 1NS,hi 7.5NS,hi 8.5NS,lo 15NS lo R
V2 A[0] gnd PWL (0NS,hi 1NS,lo 15.0NS,lo 16.0NS,hi 30NS hi R
V3 A[1] gnd PWL (0NS,hi 1NS,lo 15.0NS,lo 16.0NS,hi 30NS hi R
V4 B[0] gnd PWL (0NS,hi 1NS,lo 30.0NS,lo 31.0NS,hi 60NS hi
V5 B[1] gnd PWL (0NS,hi 1NS,lo 30.0NS,lo 31.0NS,hi 60NS hi
UC carry-in VLD2A VHD2A D2A SIGNAME=1 IS=0
UA[0] A[0] VLD2A VHD2A D2A SIGNAME=2 IS=1
UA[1] A[1] VLD2A VHD2A D2A SIGNAME=3 IS=1
UB[0] B[0] VLD2A VHD2A D2A SIGNAME=4 IS=1
UB[1] B[1] VLD2A VHD2A D2A SIGNAME=5 IS=1
0 1:1 0:2 0:3 0:4 0:5
75 0:1
150 1:1 1:2 1:3
225 0:1
300 1:1 0:2 0:3 1:4 1:5
375 0:1
450 1:1 1:2 1:3
525 0:1
600 1:1 0:2 0:3 0:4 0:5
Example
The following is an example of replacing sources with digital inputs. This
example is based on demonstration netlist digin.sp, which is available in
directory $<installdir>/demo/hspice/cchar:
* EXAMPLE OF U-ELEMENT DIGITAL OUTPUT
.OPTION POST
VOUT carry_out GND PWL 0N 0V 10N 0V 11N 5V 19N 5V 20N 0V
+ 30N 0V 31N 5V 39N 5V 40N 0V
VREF REF GND DC 0.0V
UCO carry_out REF A2D SIGNAME=12
R1 REF 0 1k
* DEFAULT DIGITAL OUTPUT MODEL (no "X" value)
206
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Replacing Sources With Digital Inputs
.MODEL A2D U LEVEL=4 TIMESTEP=0.1NS TIMESCALE=1
+ S0NAME=0 S0VLO=-1 S0VHI= 2.7
+ S4NAME=1 S4VLO= 1.4 S4VHI=9.0
+ CLOAD=0.05pf
.TRAN 1N 500N
.END
The digital output file should look something like this:
12
0
105
197
305
397
0:1
1:1
0:1
1:1
0:1
■
12 represents the signal name
■
The first column is the time, in units of 0.1 nanoseconds.
■
The second column has the signal value:name pairs.
■
This file uses more columns to represent subsequent outputs.
Also, this example based on demonstration netlist tdgt1.sp, which is available in
directory $<installdir>/demo/hspice/cchar:
*file: mos2bit.sp - adder - 2 bit all-nand-gate binary adder
*
.options post nomod fast scale=1u gmindc=100n
+
.param lmin=1.25 hi=2.8v lo=.4v vdd=4.5
.global vdd
.tran .5ns 60ns
.meas prop-delay trig v(carry-in) td=10ns val='vdd*.5' rise=1
+ targ v(c[1]) td=10ns val='vdd*.5' rise=3
*
.meas pulse-width trig v(carry-out_1) val='vdd*.5' rise=1
+ targ v(carry-out_1) val='vdd*.5' fall=1
*
.meas fall-time trig v(c[1]) td=32ns val='vdd*.9' fall=1
+ targ v(c[1]) td=32ns val='vdd*.1' fall=1
vdd vdd gnd dc vdd
x1 a[0] b[0] carry-in c[0] carry-out_1 onebit
x2 a[1] b[1] carry-out_1 c[1] carry-out_2 onebit
HSPICE® Simulation and Analysis User Guide
Y-2006.03
207
Chapter 5: Sources and Stimuli
Replacing Sources With Digital Inputs
*** subcircuit definitions
.subckt nand in1 in2 out wp=10
m1 out in1 vdd vdd p w=wp
m2 out in2 vdd vdd p w=wp
m3 out in1 mid gnd n w=wn
m4 mid in2 gnd gnd n w=wn
cload out gnd 'wp*5.7f'
.ends
wn=5
l=lmin
l=lmin
l=lmin
l=lmin
ad=0
ad=0
as=0
ad=0
.subckt onebit in1 in2 carry-in out carry-out
x1 in1 in2 #1_nand nand
x2 in1 #1_nand 8 nand
x3 in2 #1_nand 9 nand
x4 8 9 10 nand
x5 carry-in 10 half1 nand
x6 carry-in half1 half2 nand
x7 10 half1 13 nand
x8 half2 13 out nand
x9 half1 #1_nand carry-out nand
.ends onebit
* stimulus
* carryin:
* ___ ___ ___ ___
*\___/ \___/ \___/ \___/
* a register inputs:
* _______ _______
*\_______/ \_______/
* b register inputs:
* _______________
*\_______________/
*v1
*v2
*v3
*v4
*v5
carry-in
a[0] gnd
a[1] gnd
b[0] gnd
b[1] gnd
gnd
pwl
pwl
pwl
pwl
pwl(0ns,lo 1ns,hi 7.5ns,hi 8.5ns,lo 15ns lo r
(0ns,hi 1ns,lo 15.0ns,lo 16.0ns,hi 30ns hi r
(0ns,hi 1ns,lo 15.0ns,lo 16.0ns,hi 30ns hi r
(0ns,hi 1ns,lo 30.0ns,lo 31.0ns,hi 60ns hi
(0ns,hi 1ns,lo 30.0ns,lo 31.0ns,hi 60ns hi
*1 2 3 4 5
*0 1:1 0:2 0:3 0:4 0:5
*75 0:1
*150 1:1 1:2 1:3
*225 0:1
208
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Replacing Sources With Digital Inputs
*300
*375
*450
*525
*600
1:1 0:2 0:3 1:4 1:5
0:1
1:1 1:2 1:3
0:1
1:1 0:2 0:3 0:4 0:5
uc carry-in vld2a vhd2a d2a signame=1 is=0
ua[0] a[0] vld2a vhd2a d2a signame=2 is=1
ua[1] a[1] vld2a vhd2a d2a signame=3 is=1
ub[0] b[0] vld2a vhd2a d2a signame=4 is=1
ub[1] b[1] vld2a vhd2a d2a signame=5 is=1
uc0
uc1
uco
uci
c[0] vrefa2d a2d signame=10
c[1] vrefa2d a2d signame=11
carry-out_2 vrefa2d a2d signame=12
carry-in vrefa2d a2d signame=13
* models
.model n nmos level=3 vto=0.7 uo=500 kappa=.25 kp=30u
+ eta=.01 theta=.04 vmax=2e5 nsub=9e16 tox=400 gamma=1.5
+ pb=0.6 js=.1m xj=0.5u ld=0.1u nfs=1e11 nss=2e10
+ rsh=80 cj=.3m mj=0.5 cjsw=.1n mjsw=0.3
+ acm=2 capop=4
*
.model p pmos level=3 vto=-0.8 uo=150 kappa=.25 kp=15u
+ eta=.015 theta=.04 vmax=5e4 nsub=1.8e16 tox=400 gamma=.672
+ pb=0.6 js=.1m xj=0.5u ld=0.15u nfs=1e11 nss=2e10
+ rsh=80 cj=.3m mj=0.5 cjsw=.1n mjsw=0.3
+ acm=2 capop=4
*
* default digital input interface model
.model d2a u level=5 timestep=0.1ns,
+ s0name=0 s0tsw=1ns s0rlo = 15, s0rhi = 10k,
+ s2name=x s2tsw=5ns s2rlo = 1k, s2rhi = 1k
+ s3name=z s3tsw=5ns s3rlo = 1meg,s3rhi = 1meg
+ s4name=1 s4tsw=1ns s4rlo = 10k, s4rhi = 60
vld2a vld2a 0 dc lo
vhd2a vhd2a 0 dc hi
* default digital output model (no "x" value)
.model a2d u level=4 timestep=0.1ns timescale=1
+ s0name=0 s0vlo=-1 s0vhi= 2.7
+ s4name=1 s4vlo= 1.4 s4vhi=6.0
+ cload=0.05pf
vrefa2d vrefa2d 0 dc 0.0v
.end
HSPICE® Simulation and Analysis User Guide
Y-2006.03
209
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
See the plot in Figure 27 on page 210.
In this example, a 2-bit MOS adder uses a digital input file. In the plot, the
a[0], a[1], b[0], b[1], and carry-in nodes all originate from a digital file
input similar to Figure 26 on page 206. HSPICE or HSPICE RF outputs a digital
file.
Figure 27
Digital Stimulus File Input
Specifying a Digital Vector File
You can call a digital vector (VEC) file from an HSPICE netlist or from HSPICE
RF. A VEC file consists of three parts:
210
■
Vector Pattern Definition section
■
Waveform Characteristics section
■
Tabular Data section
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
To incorporate this information into your simulation, include the .VEC command
in your netlist.
Commands in a Digital Vector File
For descriptions of all commands that you can use in a VEC file, see the
“Commands in Digital Vector Files” chapter in the HSPICE Command
Reference.
Vector Patterns
The Vector Pattern Definition section defines the vectors, their names, sizes,
signal direction, sequence or order for each vector stimulus, and so on. A
RADIX line must occur first and the other lines can appear in any order in this
section. All keywords are case-insensitive.
Here is an example Vector Pattern Definition section:
; start of Vector Pattern Definition section
RADIX 1111 1111
VNAME A B C D E F G H
IO IIII IIII
TUNIT ns
These four lines are required and appear in the first lines of a VEC file:
■
RADIX defines eight single-bit vectors.
■
VNAME gives each vector a name.
■
IO determines which vectors are inputs, outputs, or bidirectional signals. In
this example, all eight are input signals.
■
TUNIT indicates that the time unit for the tabular data to follow is in units of
nanoseconds.
For additional information about these keywords, see Defining Tabular Data on
page 211.
Defining Tabular Data
Although the Tabular Data section generally appears last in a VEC file (after the
Vector Pattern and Waveform Characteristics definitions), this chapter
describes it first to introduce the definitions of a vector.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
211
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
The Tabular Data section defines (in tabular format) the values of the signals at
specified times. Rows in the Tabular Data section must appear in chronological
order, because row placement carries sequential timing information. Its general
format is:
time1 signal1_value1 signal2_value1 signal3_value1...
time2 signal1_value2 signal2_value2 signal3_value2...
time3 signal1_value3 signal2_value3 signal3_value3...
.
.
Where timex is the specified time, and signaln_valuen is the values of specific
signals at specific points in time. The set of values for a particular signal (over
all times) is a vector, which appears as a vertical column in the tabular data and
vector table. The set of all signal1_valuen constitutes one vector.
For example,
11.0 1000 1000
20.0 1100 1100
33.0 1010 1001
This example shows that:
■
At 11.0 time units, the value for the first and fifth vectors is 1.
■
At 20.0 time units, the first, second, fifth, and sixth vectors are 1.
■
At 33.0 time units, the first, third, fifth, and eighth vectors are 1.
Input Stimuli
HSPICE or HSPICE RF converts each input signal into a PWL (piecewise
linear) voltage source, and a series resistance. Table 14 shows the legal states
for an input signal. Signal values can have any of these legal states.
Table 14
212
Legal States for an Input Signal
State
Description
0
Drive to ZERO (gnd). Resistance set to 0.
1
Drive to ONE (vdd). Resistance set to 0.
Z, z
Floating to HIGH IMPEDANCE. A TRIZ statement defines resistance
value.
X, x
Drive to ZERO (gnd). Resistance set to 0.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
Table 14
Legal States for an Input Signal (Continued)
L
Resistive drive to ZERO (gnd). An OUT or OUTZ statement defines
resistance value.
H
Resistive drive to ONE (vdd). An OUT or OUTZ statement defines resistance
value.
U, u
Drive to ZERO (gnd). Resistance set to 0.
Expected Output
HSPICE or HSPICE RF converts each output signal into a .DOUT statement in
the netlist. During simulation, HSPICE or HSPICE RF compares the actual
results with the expected output vector(s). If the states are different, an error
message appears. The legal states for expected outputs include the values
listed in Table 15.
Table 15
Legal States for an Output Signal
State
Description
0
Expect ZERO.
1
Expect ONE.
X, x
Don’t care.
U, u
Don’t care.
Z, z
Expect HIGH IMPEDANCE (don’t care). Simulation evaluates Z, z as “don’t
care”, because HSPICE or HSPICE RF cannot detect a high impedance
state.
For example,
...
IO OOOO
; start of tabular section data
11.0 1001
20.0 1100
30.0 1000
35.0 xx00
HSPICE® Simulation and Analysis User Guide
Y-2006.03
213
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
Where,
■
The first line is a comment line, because of the semicolon character.
■
The second line expects the output to be 1 for the first and fourth vectors,
while all others are expected to be low.
■
At 20 time units, HSPICE or HSPICE RF expects the first and second
vectors to be high, and the third and fourth to be low.
■
At 30 time units, HSPICE or HSPICE RF expects only the first vector to be
high, and all others low.
■
At 35 time units, HSPICE or HSPICE RF expects the output of the first two
vectors to be “don’t care”; it expects vectors 3 and 4 to be low.
Verilog Value Format
HSPICE or HSPICE RF accepts Verilog-sized format to specify numbers; for
example,
<size> ’<base format> <number>
Where:
■
<size> specifies the number of bits, in decimal format.
■
<base format> indicates:
■
•
binary (’b or ’B)
•
octal (’o or ’O)
•
hexadecimal (’h or ’H).
<number> values are combinations of the 0, 1, 2, 3, 4, 5, 6, 7, 8, 9, A, B, C,
D, E, and F characters. Depending on what base format you choose, only a
subset of these characters might be legal.
You can also use unknown values (X) and high-impedance (Z) in the
<number> field. An X or Z sets four bits in the hexadecimal base, three bits
in the octal base, or one bit in the binary base.
If the most significant bit of a number is 0, X, or Z, HSPICE or HSPICE RF
automatically extends the number (if necessary), to fill the remaining bits
with 0, X, or Z, respectively. If the most significant bit is 1, HSPICE or
HSPICE RF uses 0 to extend it.
214
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
For example,
4’b1111
12’hABx
32’bZ
8’h1
This example specifies values for:
•
4-bit signal in binary
•
12-bit signal in hexadecimal
•
32-bit signal in binary
•
8-bit signal in hexadecimal
Equivalents of these lines in non-Verilog format, are:
1111
AB xxxx
ZZZZ ZZZZ ZZZZ ZZZZ ZZZZ ZZZZ ZZZZ ZZZZ
1000 0000
Periodic Tabular Data
Tabular data is often periodic, so you do not need to specify the absolute time
at every time point. When you specify the PERIOD statement, the Tabular Data
section omits the absolute times. For more information, see Defining Tabular
Data on page 211.
For example, the PERIOD statement in the following sets the time interval to
10ns between successive lines in the tabular data. This is a shortcut when you
use vectors in regular intervals throughout the entire simulation.
RADIX 1111 1111
VNAME A B C D E F G H
IO IIII IIII
TUNIT ns
PERIOD 10
; start of vector data section
1000 1000
1100 1100
1010 1001
HSPICE® Simulation and Analysis User Guide
Y-2006.03
215
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
Waveform Characteristics
The Waveform Characteristics section defines various attributes for signals,
such as the rise or fall time, the thresholds for logic high or low, and so on. For
example,
TRISE 0.3 137F 0000
TFALL 0.5 137F 0000
VIH 5.0 137F 0000
VIL 0.0 137F 0000
The waveform characteristics are based on a bit-mask. Where:
■
The TRISE (signal rise time) setting of 0.3ns applies to the first four vectors,
but not to the last four.
■
The example does not show how many bits are in each of the first four
vectors, although the first vector is at least one bit.
■
The fourth vector is four bits, because F is hexadecimal for binary 1111.
■
All bits of the fourth vector have a rise time of 0.3ns for the constant you
defined in TUNIT. This also applies to TFALL (fall time), VIH (voltage for
logic-high inputs), and VIL (voltage for logic-low inputs).
Modifying Waveform Characteristics
The TDELAY, IDELAY, and ODELAY statements define the delay time of the
signal, relative to the absolute time of each row in the Tabular Data section.
■
TDELAY applies to the input and output delay time of input, output, and
bidirectional signals.
■
IDELAY applies to the input delay time of bidirectional signals.
■
ODELAY applies to the output delay time of bidirectional signals.
The SLOPE statement specifies the rise and fall times for the input signal. To
specify the signals to which the slope applies, use a mask.
The TFALL statement sets an input fall time for specific vectors.
The TRISE statement sets an input rise time for specific vectors.
The TUNIT statement defines the time unit.
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.
216
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
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.
The VIH statement specifies the logic-high voltage for each input signal to
which the mask applies.
The VIL statement specifies the logic-low voltage for each input signal to which
the mask applies.
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.
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.
The VOH statement specifies the logic-high voltage for each output signal to
which the mask applies.
The VOL statement specifies the logic-low voltage for each output signal to
which the mask applies.
Using the Context-Based Control Option
The OPTION CBC (Context-Based Control) specifies the direction of
bidirectional signals. A bidirectional signal is an input if its value is 0, 1, or Z;
conversely, a bidirectional signal is an output if its value is H, L, U, or X.
For example,
RADIX 1 1 1
IO I O B
VNAME A Z B
OPTION CBC
10.0 0 X L
20.0 1 1 H
30.0 1 0 Z
This example sets up three vectors, named A, Z, and B. Vector A is an input,
vector Z is an output, and vector B is a bidirectional signal (defined in the IO
statement).
The OPTION CBC line turns on context-based control. The next line sets vector
A to a logic-low at 10.0 ns, and vector Z is "do not care." Because the L value
is under vector B, HSPICE expects a logic-low output.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
217
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
At 20 ns, vector A transitions high, and the expected outputs at vectors Z and B
are high. Finally, at 30 ns, HSPICE expects vector Z to be low, vector B
changes from an output to a high-impedance input, and vector the A signal
does not change.
Comment Lines and Line Continuations
Any line in a VEC file that begins with a semicolon (;) is a comment line.
Comments can also start at any point along a line. HSPICE or HSPICE RF
ignores characters after a semicolon. For example,
; This is a comment line
radix 1 1 4 1234 ; This is a radix line
As in netlists, any line in a VEC file that starts with a plus sign (+) is a
continuation from the previous line.
Parameter Usage
You can use .PARAM statements with some VEC statements when you run
HSPICE. These VEC statements fall into the three groups, which are described
in the following sections. No other VEC statements but those identified here
support .PARAM statements.
First Group
■
PERIOD
■
TDELAY
■
IDELAY
■
ODELAY
■
SLOPE
■
TRISE
■
TFALL
For these statements, the TUNIT statement defines the time unit. If you do not
include a TUNIT statement, the default time unit value is ns.
Do not specify absolute unit values in a .PARAM statement. For example, if in
your netlist:
.param myperiod=10ns
218
$ ‘ns’ makes this incorrect
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
And in your VEC file:
tunit ns
period myperiod
What you wanted for the time period is 10ns; however, because you specified
absolute units, 1e-8ns is the value used. In this example, the correct form is:
.param myperiod=10
Second Group
■
OUT or OUTZ
■
TRIZ
In these statements, the unit is ohms.
■
If you do not include an OUT (or OUTZ) statement, the default is 0.
■
If you do not include a TRIZ statement, the default is 1000M.
The .PARAM definition for this group follows the HSPICE syntax.
For example, if in your netlist:
.param myout=10
$ means 10 ohm
.param mytriz= 10Meg
$ means 10,000,000 ohm, don't
$ confuse Meg with M, M means 0.001
And in your VEC file:
out myout
triz mytriz
Then, HSPICE returns 10 ohm for OUT and 10,000,000 ohm for TRIZ.
Third Group
■
VIH
■
VIL
■
VOH
■
VOL
■
VTH
In these statements, the unit is volts.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
219
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
■
If you do not include an VIH statement, the default is 3.3.
■
If you do not include a VIL statement, the default is 0.0.
■
If you do not include a VOH statement, the default is 2.64.
■
If you do not include an VOL statement, the default is 0.66.
■
If you do not include an VTH statement, the default is 1.65.
Digital Vector File Example
; specifies # of bits associated with each vector
radix 1 2 444
;********************************************************
; defines name for each vector. For multi-bit vectors,
; innermost [] provide the bit index range, MSB:LSB
vname v1 va[[1:0]] vb[12:1]
;actual signal names: v1, va[0], va[1], vb1, vb2, ... vb12
;********************************************************
; defines vector as input, output, or bi-directional
io i o bbb
; defines time unit
tunit ns
;********************************************************
; vb12-vb5 are output when ‘v1’ is ‘high’
enable v1 0 0 FF0
; vb4-vb1 are output when ‘v1’ is ‘low’
enable ~v1 0 0 00F
;********************************************************
; all signals have a delay of 1 ns
; Note: do not put the unit (such as ns) here again.
; HSPICE multiplies this value by the specified ‘tunit’.
tdelay 1.0
; va1 and va0 signals have 1.5ns delays
tdelay 1.5 0 3 000
;********************************************************
; specify input rise/fall times (if you want different
; rise/fall times, use the trise/tfall statement.)
; Note: do not put the unit (such as ns) here again.
; HSPICE multiplies this value by the specified ‘tunit’.
slope 1.2
;********************************************************
; specify the logic ‘high’ voltage for input signals
vih 3.3 1 0 000
vih 5.0 0 0 FFF
; to specify logic low, use ‘vil’
;********************************************************
220
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
; va & vb switch from ‘lo’ to ‘hi’ at 1.75 volts
vth 1.75 0 1 FFF
;****************************************************
; tabular data section
10.0 1 3 FFF
20.0 0 2 AFF
30.0 1 0 888
HSPICE® Simulation and Analysis User Guide
Y-2006.03
221
Chapter 5: Sources and Stimuli
Specifying a Digital Vector File
222
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Using Parameters in Simulation (.PARAM)
6
6
Parameters and Functions
Describes how to use parameters within an HSPICE netlist.
Parameters are similar to the variables used in most programming languages.
Parameters hold a value that you assign when you create your circuit design or
that the simulation calculates based on circuit solution values. Parameters can
store static values for a variety of quantities (resistance, source voltage, rise
time, and so on). You can also use them in sweep or statistical analysis.
For descriptions of individual HSPICE commands referenced in this chapter,
see the “Netlist Commands” chapter in the HSPICE Command Reference.
Using Parameters in Simulation (.PARAM)
Defining Parameters
Parameters in HSPICE are names that you associate with numeric values.
(See Assigning Parameters on page 225.) You can use any of the methods
described in Table 16 to define parameters.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
223
Chapter 6: Parameters and Functions
Using Parameters in Simulation (.PARAM)
Table 16
.PARAM Statement Syntax
Parameter
Description
Simple assignment
.PARAM <SimpleParam>=1e-12
Algebraic definition
.PARAM <AlgebraicParam>=‘SimpleParam*8.2’
SimpleParam excludes the output variable.
You can also use algebraic parameters in .PRINT and .PROBE
statements (HSPICE or HSPICE RF), and in .PLOT, and .GRAPH
statements (HSPICE only). For example:
.PRINT AlgebraicParam=par(’algebraic expression’)
You can use the same syntax for .PROBE, .PLOT, and .GRAPH
statements. See Using Algebraic Expressions on page 228.
User-defined function
.PARAM <MyFunc( x, y )>=‘Sqrt((x*x)+(y*y))’
Character string
definition
.PARAM <paramname>=str(‘string’)
Subcircuit default
.SUBCKT <SubName> <ParamDefName>=<Value> str(‘string’)
.MACRO <SubName> <ParamDefName>=<Value> str(‘string’)
Predefined analysis
function
.PARAM <mcVar>=Agauss(1.0,0.1)
.MEASURE statement
.MEASURE <DC | AC | TRAN> result TRIG ...
+ TARG ... <GOAL=val> <MINVAL=val>
+ <WEIGHT=val> <MeasType> <MeasParam>
(See Specifying User-Defined Analysis (.MEASURE) on page 267.)
.PRINT | .PROBE |
.PLOT | .GRAPH
.PRINT | .PROBE | .PLOT | .GRAPH <DC|AC|TRAN>
+ outParam=Par_Expression
A parameter definition in HSPICE always uses the last value found in the input
netlist (subject to local versus global parameter rules). The definitions below
assign a value of 3 to the DupParam parameter.
.PARAM DupParam=1
...
.PARAM DupParam=3
224
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Using Parameters in Simulation (.PARAM)
HSPICE assigns 3 as the value for all instances of DupParam, including
instances that are earlier in the input than the .PARAM DupParam=3
statement.
All parameter values in HSPICE are IEEE double floating point numbers. The
parameter resolution order is:
1. Resolve all literal assignments.
2. Resolve all expressions.
3. Resolve all function calls.
Table 17 shows the parameter passing order.
Table 17
Parameter Passing Order
.OPTION PARHIER=GLOBAL
.OPTION PARHIER=LOCAL
Analysis sweep parameters
Analysis sweep parameters
.PARAM statement (library)
.SUBCKT call (instance)
.SUBCKT call (instance)
.SUBCKT definition (symbol)
.SUBCKT definition (symbol)
.PARAM statement (library)
Assigning Parameters
You can assign the following types of values to parameters:
■
Constant real number
■
Algebraic expression of real values
■
Predefined function
■
Function that you define
■
Circuit value
■
Model value
To invoke the algebraic processor, enclose a complex expression in single
quotes. A simple expression consists of one parameter name.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
225
Chapter 6: Parameters and Functions
Using Parameters in Simulation (.PARAM)
The parameter keeps the assigned value, unless:
■
A later definition changes its value, or
■
An algebraic expression assigns a new value during simulation.
HSPICE does not warn you, if it reassigns a parameter.
Inline Parameter Assignments
To define circuit values, using a direct algebraic evaluation:
r1 n1 0 R=’1k/sqrt(HERTZ)’ $ Resistance for frequency
Parameters in Output
To use an algebraic expression as an output variable in
a .PRINT, .PLOT, .PROBE .GRAPH, or .MEASURE statement, use the PAR
keyword. (See Chapter 7, Simulation Output, for more information.)
Example
.PRINT DC v(3) gain=PAR(‘v(3)/v(2)’) PAR(‘v(4)/v(2)’)
User-Defined Function Parameters
You can define a function that is similar to the parameter assignment, but you
cannot nest the functions more than two deep.
■
An expression can contain parameters that you did not define.
■
A function must have at least one argument, and can have up to 20 (and in
many cases, more than 20) arguments.
■
You can redefine functions.
The format of a function is:
funcname1(arg1[,arg2...])=expression1
+ [funcname2(arg1[,arg2...])=expression2] off
226
Parameter
Description
funcname
Specifies the function name. This parameter must be distinct from
array names and built-in functions. In subsequently defined functions,
all embedded functions must be previously defined.
arg1, arg2
Specifies variables used in the expression.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Using Parameters in Simulation (.PARAM)
Parameter
Description
off
Voids all user-defined functions.
Example
.PARAM f(a,b)=POW(a,2)+a*b g(d)=SQRT(d)
+ h(e)=e*f(1,2)-g(3)
Predefined Analysis Function
HSPICE includes specialized analysis types, such as Optimization and Monte
Carlo, that require a way to control the analysis.
Measurement Parameters
.MEASURE statements produce a measurement parameter. The rules for
measurement parameters are the same as for standard parameters, except
that measurement parameters are defined in a .MEASURE statement, not in
a .PARAM statement. For a description of the .MEASURE statement, see
Specifying User-Defined Analysis (.MEASURE) on page 267.
.PRINT, .PROBE, .PLOT, and .GRAPH Parameters
.PRINT,.PROBE,.PLOT, and .GRAPH statements in HSPICE produce a print
parameter. The rules for print parameters are the same as the rules for
standard parameters, except that you define the parameter directly in
a.PRINT,.PROBE,.PLOT, or .GRAPH statement, not in a .PARAM statement.
HSPICE RF does not support .PLOT or .GRAPH statements.
For more information about the.PRINT,.PROBE,.PLOT, or .GRAPH
statements, see Displaying Simulation Results on page 243.
Multiply Parameter
The most basic subcircuit parameter in HSPICE is the M (multiply) parameter.
For a description of this parameter, see M (Multiply) Parameter on page 58.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
227
Chapter 6: Parameters and Functions
Using Algebraic Expressions
Using Algebraic Expressions
Note:
Synopsys HSPICE uses double-precision numbers (15 digits) for
expressions, user-defined parameters, and sweep variables. For better
precision, use parameters (instead of constants) in algebraic expressions,
because constants are only single-precision numbers (7 digits).
In HSPICE, an algebraic expression, with quoted strings, can replace any
parameter in the netlist.
In HSPICE, you can then use these expressions as output variables
in .PLOT, .PRINT, and .GRAPH statements. Algebraic expressions can
expand your options in an input netlist file.
Some uses of algebraic expressions are:
■
Parameters:
.PARAM x=’y+3’
■
Functions:
.PARAM rho(leff,weff)=’2+*leff*weff-2u’
■
Algebra in elements:
R1 1 0 r=’ABS(v(1)/i(m1))+10’
■
Algebra in .MEASURE statements:
.MEAS vmax MAX V(1)
.MEAS imax MAX I(q2)
.MEAS ivmax PARAM=’vmax*imax’
■
Algebra in output statements:
.PRINT conductance=PAR(‘i(m1)/v(22)’)
The basic syntax for using algebraic expressions for output is:
PAR(‘algebraic expression’)
In addition to using quotations, you must define the expression inside the
PAR( ) statement for output.The continuation character for quoted parameter
strings, in HSPICE, is a double backslash (\\). (Outside of quoted strings, the
single backslash (\) is the continuation character.)
228
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Built-In Functions and Variables
Built-In Functions and Variables
In addition to simple arithmetic operations (+, -, *, /), you can use the built-in
functions listed in Table 18 and the variables listed in Table 17 on page 225 in
HSPICE expressions.
Table 18
Synopsys HSPICE Built-in Functions
HSPICE Form
Function
Class
Description
sin(x)
sine
trig
Returns the sine of x (radians)
cos(x)
cosine
trig
Returns the cosine of x (radians)
tan(x)
tangent
trig
Returns the tangent of x (radians)
asin(x)
arc sine
trig
Returns the inverse sine of x (radians)
acos(x)
arc cosine
trig
Returns the inverse cosine of x (radians)
atan(x)
arc tangent
trig
Returns the inverse tangent of x (radians)
sinh(x)
hyperbolic
sine
trig
Returns the hyperbolic sine of x (radians)
cosh(x)
hyperbolic
cosine
trig
Returns the hyperbolic cosine of x (radians)
tanh(x)
hyperbolic
tangent
trig
Returns the hyperbolic tangent of x (radians)
abs(x)
absolute
value
math
Returns the absolute value of x: |x|
sqrt(x)
square root
math
Returns the square root of the absolute value of x:
sqrt(-x)=-sqrt(|x|)
pow(x,y)
absolute
power
math
Returns the value of x raised to the integer part of y:
x(integer part of y)
pwr(x,y)
signed
power
math
Returns the absolute value of x, raised to the y
power, with the sign of x: (sign of x)|x|y
HSPICE® Simulation and Analysis User Guide
Y-2006.03
229
Chapter 6: Parameters and Functions
Built-In Functions and Variables
Table 18
Synopsys HSPICE Built-in Functions (Continued)
HSPICE Form
Function
x**y
power
Class
Description
If x<0, returns the value of x raised to the integer part
of y.
If x=0, returns 0.
If x>0, returns the value of x raised to the y power.
log(x)
natural
logarithm
math
Returns the natural logarithm of the absolute value of
x, with the sign of x: (sign of x)log(|x|)
log10(x)
base 10
logarithm
math
Returns the base 10 logarithm of the absolute value
of x, with the sign of x: (sign of x)log10(|x|)
exp(x)
exponential
math
Returns e, raised to the power x: ex
db(x)
decibels
math
Returns the base 10 logarithm of the absolute value
of x, multiplied by 20, with the sign of x: (sign of
x)20log10(|x|)
int(x)
integer
math
Returns the integer portion of x. The fractional
portion of the number is lost.
nint(x)
integer
math
Rounds x up or down, to the nearest integer.
sgn(x)
return sign
math
Returns -1 if x is less than 0.
Returns 0 if x is equal to 0.
Returns 1 if x is greater than 0
sign(x,y)
transfer sign math
Returns the absolute value of x, with the sign of y:
(sign of y)|x|
min(x,y)
smaller of
two args
control
Returns the numeric minimum of x and y
max(x,y)
larger of two control
args
Returns the numeric maximum of x and y
val(element)
get value
Returns a parameter value for a specified element.
For example, val(r1) returns the resistance value of
the r1 resistor.
230
various
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Built-In Functions and Variables
Table 18
Synopsys HSPICE Built-in Functions (Continued)
HSPICE Form
Function
Class
Description
val(element.
parameter)
get value
various
Returns a value for a specified parameter of a
specified element. For example, val(rload.temp)
returns the value of the temp (temperature)
parameter for the rload element.
val(model_type:
model_name.
model_param)
get value
various
Returns a value for a specified parameter of a
specified model of a specific type. For example,
val(nmos:mos1.rs) returns the value of the rs
parameter for the mos1 model, which is an nmos
model type.
lv(<Element>)
or
lx(<Element>)
element
templates
various
Returns various element values during simulation.
See Element Template Output on page 266 for more
information.
v(<Node>),
i(<Element>)...
circuit
output
variables
various
Returns various circuit values during simulation. See
DC and Transient Output Variables on page 251 for
more information.
[cond] ?x : y
ternary
operator
Returns x if cond is not zero. Otherwise, returns y.
relational
operator
(less than)
Returns 1 if the left operand is less than the right
operand. Otherwise, returns 0.
relational
operator
(less than or
equal)
Returns 1 if the left operand is less than or equal to
the right operand. Otherwise, returns 0.
relational
operator
(greater
than)
Returns 1 if the left operand is greater than the right
operand. Otherwise, returns 0.
<
<=
>
HSPICE® Simulation and Analysis User Guide
Y-2006.03
.param z=’condition ? x:y’
.para x=y<z (y less than z)
.para x=y<=z (y less than or equal to z)
.para x=y>z (y greater than z)
231
Chapter 6: Parameters and Functions
Built-In Functions and Variables
Table 18
Synopsys HSPICE Built-in Functions (Continued)
HSPICE Form
Function
>=
relational
operator
(greater
than or
equal)
Returns 1 if the left operand is greater than or equal
to the right operand. Otherwise, returns 0.
equality
Returns 1 if the operands are equal. Otherwise,
returns 0.
==
Class
Description
.para x=y>=z (y greater than or equal to z)
.para x=y==z (y equal to z)
!=
inequality
Returns 1 if the operands are not equal. Otherwise,
returns 0.
.para x=y!=z (y not equal to z)
&&
Logical
AND
Returns 1 if neither operand is zero. Otherwise,
returns 0. .para x=y&&z (y AND z)
||
Logical OR
Returns 1 if either or both operands are not zero.
Returns 0 only if both operands are zero.
.para x=y||z (y OR z)
Example
.parameters p1=4 p2=5 p3=6
r1 1 0 value='p1 ? p2+1 : p3'
HSPICE reserves the variable names listed in Table 19 on page 232 for use in
elements, such as E, G, R, C, and L. You can use them in expressions, but you
cannot redefine them; for example, this statement would be illegal:
.param temper=100
Table 19
Synopsys HSPICE Special Variables
HSPICE Form
Function
Class
Description
time
current
simulation
time
control
Uses parameters to define the current simulation
time, during transient analysis.
232
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
Table 19
Synopsys HSPICE Special Variables (Continued)
HSPICE Form
Function
Class
Description
temper
current circuit
temperature
control
Uses parameters to define the current simulation
temperature, during transient/temperature
analysis.
hertz
current
simulation
frequency
control
Uses parameters to define the frequency, during
AC analysis.
Parameter Scoping and Passing
If you use parameters to define values in sub-circuits, you need to create fewer
similar cells, to provide enough functionality in your library. You can pass circuit
parameters into hierarchical designs, and assign different values to the same
parameter within individual cells, when you run simulation.
For example, if you use parameters to set the initial state of a latch in its
subcircuit definition, then you can override this initial default in the instance call.
You need to create only one cell, to handle both initial state versions of the
latch.
You can also use parameters to define the cell layout. For example, you can
use parameters in a MOS inverter, to simulate a range of inverter sizes, with
only one cell definition. Local instances of the cell can assign different values to
the size parameter for the inverter.
In HSPICE, you can also perform Monte Carlo analysis or optimization on a cell
that uses parameters.
How you handle hierarchical parameters depends on how you construct and
analyze your cells. You can construct a design in which information flows from
the top of the design, down into the lowest hierarchical levels.
■
To centralize the control at the top of the design hierarchy, set global
parameters.
■
To construct a library of small cells that are individually controlled from
within, set local parameters and build up to the block level.
This section describes the scope of parameter names, and how HSPICE
resolves naming conflicts between levels of hierarchy.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
233
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
Library Integrity
Integrity is a fundamental requirement for any symbol library. Library integrity
can be as simple as a consistent, intuitive name scheme, or as complex as
libraries with built-in range checking.
Library integrity might be poor if you use libraries from different vendors in a
circuit design. Because names of circuit parameters are not standardized
between vendors, two components can include the same parameter name for
different functions. For example, one vendor might build a library that uses the
name Tau as a parameter to control one or more subcircuits in their library.
Another vendor might use Tau to control a different aspect of their library. If you
set a global parameter named Tau to control one library, you also modify the
behavior of the second library, which might not be the intent.
If the scope of a higher-level parameter is global to all subcircuits at lower levels
of the design hierarchy, higher-level definitions override lower-level parameter
values with the same names. The scope of a lower-level parameter is local to
the subcircuit where you define the parameter (but global to all subcircuits that
are even lower in the design hierarchy). Local scoping rules in HSPICE prevent
higher-level parameters from overriding lower-level parameters of the same
name, when that is not desired.
Reusing Cells
Parameter name problems also occur if different groups collaborate on a
design. Global parameters prevail over local parameters, so all circuit
designers must know the names of all parameters, even those used in sections
of the design for which they are not responsible. This can lead to a large
investment in standard libraries. To avoid this situation, use local parameter
scoping, to encapsulate all information about a section of a design, within that
section.
Creating Parameters in a Library
To ensure that the input netlist includes critical, user-supplied parameters when
you run simulation, you can use “illegal defaults”—that is, defaults that cause
the simulator to abort if you do not supply overrides for the defaults.
If a library cell includes illegal defaults, you must provide a value for each
instance of those cells. If you do not, the simulation aborts.
234
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
For example, you might define a default MOSFET width of 0.0. HSPICE aborts,
because MOSFET models require this parameter.
Example 1
* Subcircuit default definition
.SUBCKT Inv A Y Wid=0 $ Inherit illegal values by default
mp1 <NodeList> <Model> L=1u W=’Wid*2’
mn1 <NodeList> <Model> L=1u W=Wid
.ENDS
* Invoke symbols in a design
x1 A Y1 Inv
$ Bad! No widths specified
x2 A Y2 Inv Wid=1u $ Overrides illegal value for Width
This simulation aborts on the x1 subcircuit instance, because you never set the
required Wid parameter on the subcircuit instance line. The x2 subcircuit
simulates correctly. Additionally, the instances of the Inv cell are subject to
accidental interference, because the Wid global parameter is exposed outside
the domain of the library. Anyone can specify an alternative value for the
parameter, in another section of the library or the circuit design. This might
prevent the simulation from catching the condition on x1.
Example 2
In this example, the name of a global parameter conflicts with the internal
library parameter named Wid. Another user might specify such a global
parameter, in a different library. In this example, the user of the library has
specified a different meaning for the Wid parameter, to define an independent
source.
.Param Wid=5u
$ Default Pulse Width for source
v1 Pulsed 0 Pulse ( 0v 5v 0u 0.1u 0.1u Wid 10u )
...
* Subcircuit default definition
.SUBCKT Inv A Y Wid=0
$ Inherit illegals by default
mp1 <NodeList> <Model> L=1u W=’Wid*2’
mn1 <NodeList> <Model> L=1u W=Wid
.Ends
* Invoke symbols in a design
x1 A Y1 Inv
$ Incorrect width!
x2 A Y2 Inv Wid=1u
$ Incorrect! Both x1 and x2
$ simulate with mp1=10u and
$ mn1=5u instead of 2u and 1u.
Under global parameter scoping rules, simulation succeeds, but incorrectly.
HSPICE does not warn you that the x1 inverter has no assigned width,
because the global parameter definition for Wid overrides the subcircuit default.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
235
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
Note:
Similarly, sweeping with different values of Wid dynamically changes both
the Wid library internal parameter value, and the pulse width value to the
Wid value of the current sweep.
In global scoping, the highest-level name prevails, when resolving name
conflicts. Local scoping uses the lowest-level name.
When you use the parameter inheritance method, you can specify to use local
scoping rules. This feature can cause different results than you obtained using
HSPICE versions before release 95.1, on existing circuits.
When you use local scoping rules, the Example 2 netlist correctly aborts in x1
for W=0 (default Wid=0, in the .SUBCKT definition, has higher precedence,
than the .PARAM statement). This results in the correct device sizes for x2. This
change can affect your simulation results, if you intentionally or accidentally
create a circuit such as the second one shown above.
As an alternative to width testing in the Example 2 netlist, you can
use .OPTION DEFW to achieve a limited version of library integrity. This option
sets the default width for all MOS devices during a simulation. Part of the
definition is still in the top-level circuit, so this method can still make unwanted
changes to library values, without notification from the HSPICE simulator.
Table 20 compares the three primary methods for configuring libraries, to
achieve required parameter checking for default MOS transistor widths.
Table 20
Method
Methods for Configuring Libraries
Parameter
Location
Pros
Cons
Local
On a .SUBCKT
definition line
Protects library from global
circuit parameter definitions,
unless you override it. Single
location for default values.
You cannot use it with versions
of HSPICE before Release
95.1.
Global
At the global level
and on .SUBCKT
definition lines
Works with older HSPICE
versions.
An indiscreet user, another
vendor assignment, or the
intervening hierarchy can
change the library. Cannot
override a global value at a
lower level.
236
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
Table 20
Methods for Configuring Libraries (Continued)
Parameter
Location
Method
Special
.OPTION DEFW
statement
Pros
Cons
Simple to do.
Third-party libraries, or other
sections of the design, might
depend on .OPTION DEFW.
String Parameter
HSPICE uses a special delimiter to identify string and double parameter types.
The single quotes (‘), double quotes (“), or curly brackets ( {} ) do not work for
these kinds of delimiters. Instead, use the sp1=str('string') keyword for an sp1
parameter definition and use the str(sp1) keyword for a string parameter
instance.
Example
The following sample netlist shows an example of how you can use these
definitions for various commands, keywords, parameters, and elements:
xibis1 vccq vss out in IBIS
+ IBIS_FILE=str('file1.ibs') IBIS_MODEL=str('model1')
xibis2 vccq vss out in IBIS
+ IBIS_FILE=str('file2.ibs') IBIS_MODEL=str('model2')
.subckt IBIS vccq vss out in
+ IBIS_FILE=str('file.ibs')
+ IBIS_MODEL=str('ibis_model')
ven en 0 vcc
BMCH vccq vss out in en v0dq0 vccq vss buffer=3
+ file= str(IBIS_FILE) model=str(IBIS_MODEL)
+ typ=typ ramp_rwf=2 ramp_fwf=2 power=on
.ends
HSPICE can now support these kinds of definitions and instances with the
following netlist components:
■
.PARAM statements
■
.SUBCKT statements
■
FQMODEL keywords
■
S Parameters
■
FILE and MODEL keywords
HSPICE® Simulation and Analysis User Guide
Y-2006.03
237
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
■
B Elements
■
RLGCFILE, UMODEL, FSMODEL, RLGCMODEL, TABLEMODEL, and SMODEL
keywords in the W Element
Parameter Defaults and Inheritance
Use the .OPTION PARHIER parameter to specify scoping rules.
Syntax:
.OPTION PARHIER=< GLOBAL | LOCAL >
The default setting is GLOBAL.
Example
This example explicitly shows the difference between local and global scoping
for using parameters in subcircuits.
The input netlist includes the following:
.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
Set the .OPTION PARHIER=parameter scoping option to GLOBAL. The
netlist also includes the following input statements:
xInv0 a y0 Inv
$ override DefPwid default,
$ xInv0.Mp1 width=1u
xInv1 a y1 Inv DefPwid=5u $ override DefPwid=5u,
$ xInv1.Mp1 width=1u
.measure tran Wid0 param=’lv2(xInv0.Mp1)’ $ lv2 is the
$ template for
.measure tran Wid1 param=’lv2(xInv1.Mp1)’ $ the channel
$ width
$ ‘lv2(xInv1.Mp1)’
.ENDS
Simulating this netlist produces the following results in the listing file:
wid0=1.0000E-06
wid1=1.0000E-06
238
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
If you change the .OPTION PARHIER=parameter scoping option
to LOCAL:
xInv0 a y0 Inv
$ not override .param
$ DefPwid=2u,
$ xInv0.Mp1 width=2u
xInv1 a y1 Inv DefPwid=5u
$ override .param
$ DefPwid=2u,
$ xInv1.Mp1 width=5u:
.measure tran Wid0 param=’lv2(xInv0.Mp1)’$ override the
.measure tran Wid1 param=’lv2(xInv1.Mp1)’$ global .PARAM
...
Simulation produces the following results in the listing file:
wid0=2.0000E-06
wid1=5.0000E-06
Parameter Passing
Figure 28 on page 239 shows a flat representation of a hierarchical circuit,
which contains three resistors.
Each of the three resistors obtains its simulation time resistance from the Val
parameter. The netlist defines the Val parameter in four places, with three
different values.
Figure 28
+
Hierarchical Parameter Passing Problem
Sub1
Sub2
Sub3
r1
r2
r3
1V
-
HSPICE® Simulation and Analysis User Guide
Y-2006.03
TEST OF PARHIER
.OPTION list node post=2
+ ingold=2
+ parhier=<Local|Global>
.PARAM Val=1
x1 n0 0 Sub1
.SubCkt Sub1 n1 n2 Val=1
r1 n1 n2 Val
x2 n1 n2 Sub2
.Ends Sub1
.SubCkt Sub2 n1 n2 Val=2
r2 n1 n2 Val
x3 n1 n2 Sub3
.Ends Sub2
.SubCkt Sub3 n1 n2 Val=3
r3 n1 n2 Val
.Ends Sub3
.OP
.END
239
Chapter 6: Parameters and Functions
Parameter Scoping and Passing
The total resistance of the chain has two possible solutions: 0.3333Ω and
0.5455Ω.
You can use .OPTION PARHIER to specify which parameter value prevails,
when you define parameters with the same name at different levels of the
design hierarchy.
Under global scoping rules, if names conflict, the top-level assignment .PARAM
Val=1 overrides the subcircuit defaults, and the total is 0.3333Ω. Under local
scoping rules, the lower level assignments prevail, and the total is 0.5455Ω
(one, two, and three ohms in parallel).
The example in Figure 28 produces the results in Table 21, based on how you
set .OPTION PARHIER to local/global:
Table 21
PARHIER=LOCAL vs. PARHIER=GLOBAL Results
Element
PARHIER=Local
PARHIER=Global
r1
1.0
1.0
r2
2.0
1.0
r3
3.0
1.0
Parameter Passing Solutions
Changes in scoping rules can cause different simulation results for circuit
designs created before HSPICE Release 95.1, than for designs created after
that release. The checklist below determines whether you will see simulation
differences when you use the new default scoping rules. These checks are
especially important if your netlists contain devices from multiple vendor
libraries.
240
■
Check your sub-circuits for parameter defaults, on the .SUBCKT or .MACRO
line.
■
Check your sub-circuits for a .PARAM statement, within a .SUBCKT
definition.
■
To check your circuits for global parameter definitions, use the .PARAM
statement.
■
If any of the names from the first three checks are identical, set up two
HSPICE simulation jobs: one with .OPTION PARHIER=GLOBAL, and one
with .OPTION PARHIER=LOCAL. Then look for differences in the output.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Overview of Output Statements
7
7
Simulation Output
Describes how to use output format statements and variables to display steady
state, frequency, and time domain simulation results.
You can also use output variables in behavioral circuit analysis, modeling, and
simulation techniques. To display electrical specifications such as rise time,
slew rate, amplifier gain, and current density, use the output format features.
For descriptions of individual HSPICE commands referenced in this chapter,
see the HSPICE Command Reference.
Overview of Output Statements
Output Commands
The input netlist file contains output statements, including .PRINT,
.PLOT, .GRAPH, .PROBE, .MEASURE, .DOUT, and .STIM. Each statement
specifies the output variables, and the type of simulation result, to display—
such as .DC, .AC, or .TRAN. When you specify .OPTION POST, Synopsys
HSPICE puts all output variables, referenced in .PRINT, .PLOT, .GRAPH,
.PROBE, .MEASURE, .DOUT, and .STIM statements into HSPICE output files.
HSPICE RF supports only .OPTION POST, .OPTION PROBE, .PRINT,
.PROBE, and .MEASURE statements. It does not support .DOUT, .PLOT,
.GRAPH, or .STIM statements. CosmosScope provides high-resolution, postsimulation, and interactive display of waveforms.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
241
Chapter 7: Simulation Output
Overview of Output Statements
Table 22
Output Statements
Output
Statement
Description
.PRINT
Prints numeric analysis results in the output listing file (and postprocessor data, if you specify .OPTION POST).
.PLOT (HSPICE
only)
Obsolete option. Use .PRINT or ..PROBE to generate necessary
plot in the output listing file. Generates low-resolution (ASCII) plots
in the output listing file (and post-processor data, if you
specify .OPTION POST), in HSPICE only (not supported in
HSPICE RF).
.GRAPH
(HSPICE only)
Obsolete option. Use .PRINT or ..PROBE to generate necessary
plot in the output listing file. Generates high-resolution plots for
specific printing devices (such as HP LaserJet), or in PostScript
format (intended for hard-copy outputs, without using a postprocessor).
.PROBE
Outputs data to post-processor output files, but not to the output
listing (used with .OPTION PROBE, to limit output).
.MEASURE
Prints the results of specific user-defined analyses (and postprocessor data, if you specify .OPTION POST), to the output
listing file. or HSPICE RF
.DOUT
Specifies the expected final state of an output signal (HSPICE
only; not supported in HSPICE RF).
.STIM (HSPICE
only)
Specifies simulation results to transform to PWL, Data Card, or
Digital Vector File format.
Output Variables
The output format statements require special output variables, to print or plot
analysis results for nodal voltages and branch currents. HSPICE or HSPICE
RF uses the following output variables:
242
■
DC and transient analysis
■
AC analysis
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Displaying Simulation Results
■
element template (HSPICE)
■
.MEASURE statement
■
parametric analysis
For HSPICE or HSPICE RF, DC and transient analysis displays:
■
individual nodal voltages: V(n1 [,n2])
■
branch currents: I(Vxx)
■
element power dissipation: In(element)
AC analysis displays imaginary and real components of a nodal voltage or
branch current, and the magnitude and phase of a nodal voltage or branch
current. AC analysis results also print impedance parameters, and input and
output noise.
Element template analysis displays element-specific nodal voltages, branch
currents, element parameters, and the derivatives of the element’s node
voltage, current, or charge.
The .MEASURE statement variables define the electrical characteristics to
measure in a .MEASURE statement analysis or HSPICE RF.
Parametric analysis variables are mathematical expressions, which operate on
nodal voltages, branch currents, element template variables (HSPICE only; not
supported in HSPICE RF), or other parameters that you specify. Use these
variables when you run behavioral analysis of simulation results. See Using
Algebraic Expressions on page 228 or HSPICE RF.
Displaying Simulation Results
The following section describes the statements that you can use to display
simulation results for your specific requirements.
.PRINT Statement
The .PRINT statement specifies output variables for which HSPICE or
HSPICE RF prints values.
■
The maximum number of variables in a single .PRINT statement, was 32
before Release 2002.2, but has been extended. For example, you can enter:
.PRINT v(1) v(2) ... v(32) v(33) v(34)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
243
Chapter 7: Simulation Output
Displaying Simulation Results
This function previously required two .PRINT statements:
.PRINT v(1) v(2) ... v(32)
.PRINT v(33) v(34)
■
To simplify parsing of the output listings, HSPICE or HSPICE RF prints a
single x in the first column, to indicate the beginning of the .PRINT output
data. A single y in the first column indicates the end of the .PRINT output
data.
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.
Example
If your circuit contains four MOSFET elements (named m1, m2, m3, m4),
then .PRINT iall (m*) is equivalent to .PRINT i(m1) i(m2) i(m3) i(m4). It prints
the output currents of all four MOSFET elements.
Statement Order
HSPICE or HSPICE RF creates different .sw0 and .tr0 files, based on the order
of the .PRINT and .DC statements. If you do not specify an analysis type for
a .PRINT command, the type matches the last analysis command in the
244
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Displaying Simulation Results
To make HSPICE find plot limits for each plot individually, use .OPTION PLIM
to create a different axis for each plot variable. The PLIM option is similar to the
plot limit algorithm in SPICE2G.6, where each plot can have limits different
from any other plot. A number from 2 through 9 indicates the overlap of two or
more traces on a plot.
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 specify an unlimited number of .PLOT statements for each type of
analysis. To set the plot width, use .OPTION CO (columns out). If you set
CO=80, the plot has 50 columns. If CO=132, the plot has 100 columns.
You can include wildcards in .PLOT statements (HSPICE only).
.PROBE Statement
HSPICE or HSPICE RF usually saves all voltages, supply currents, and output
variables. Set .OPTION PROBE, to save output variables only. Use the .PROBE
statement to specify the quantities to print in the output listing.
If you are interested only in the output data file, and you do not want tabular or
plot data in your listing file, set .OPTION PROBE and use .PROBE to select the
values to save in the output listing.
You can include wildcards in .PROBE statements.
.GRAPH Statement
Note:
This is an obsolete statement. You can gain the same functionality by using
the .PROBE statement (see .PROBE Statement on page 245).
Use the .GRAPH statement when you need high-resolution plots of HSPICE
simulation results.
Note:
You cannot use .GRAPH statements in the PC version of HSPICE, or in any
versions of HSPICE RF.
The .GRAPH statement is similar to the .PLOT statement, with the addition of
an optional model. When you specify a model, you can add or change graphing
properties for the graph. The .GRAPH statement generates a .gr# graph data
HSPICE® Simulation and Analysis User Guide
Y-2006.03
245
Chapter 7: Simulation Output
Displaying Simulation Results
file and sends this file directly to the default high resolution graphical device (to
specify this device, set PRTDEFAULT in the meta.cfg configuration file).
.MODEL Statement for .GRAPH
For a description of how to use the .MODEL statement with .GRAPH, see the
.MODEL command in the HSPICE Command Reference. HSPICE RF does not
support the .GRAPH statement.
Table 23
Model Parameters
Name (Alias)
Default
Description
MONO
0.0
Monotonic option. MONO=1 automatically resets the x-axis, if any
change occurs in the x direction.
TIC
0.0
Shows tick marks.
FREQ
0.0
Plots symbol frequency.
■
A value of 0 does not generate plot symbols.
A value of n generates a plot symbol every n points.
This is not the same as the FREQ keyword in element statements
(see the “Modeling Filters and Networks” chapter in the HSPICE
Applications Manual).
■
XGRID, YGRID
0.0
Set these values to 1.0, to turn on the axis grid lines.
XMIN, XMAX
0.0
■
■
XSCAL
1.0
If XMIN is not equal to XMAX, then XMIN and XMAX determine
the x-axis plot limits.
If XMIN equals XMAX, or if you do not set XMIN and XMAX,
then HSPICE automatically sets the plot limits. These limits
apply to the actual x-axis variable value, regardless of the
XSCAL type.
Scale for the x-axis. Two common axis scales are:
Linear(LIN)
(XSCAL=1)
Logarithm(LOG) (XSCAL=2)
246
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Displaying Simulation Results
Table 23
Model Parameters (Continued)
Name (Alias)
Default
Description
YMIN, YMAX
0.0
■
■
YSCAL
1.0
If YMIN is not equal to YMAX, then YMIN and YMAX determine
the y-axis plot limits.
The y-axis limits in the .GRAPH statement overrides YMIN and
YMAX in the model.
If you do not specify plot limits, HSPICE sets the plot limits.
These limits apply to the actual y-axis variable value,
regardless of the YSCAL type.
Scale for the y-axis. Two common axis scales are:
Linear(LIN)
(XSCAL=1)
Logarithm(LOG) (XSCAL=2)
Using Wildcards in PRINT, PROBE, PLOT, and GRAPH
Statements
You can include wildcards in .PRINT and .PROBE statements (HSPICE and
HSPICE RF), and in .PLOT and .GRAPH statements (HSPICE only). Refer to
this example netlist in the discussion that follows:
* test wildcard
.option post
v1 1 0 10
r1 1 n20 10
r20 n20 n21 10
r21 n21 0 10
.dc v1 1 10 1
***Wildcard equivalent for:
*.print i(r1) i(r20) i(r21) i(v1)
.print i(*)
***Wildcard equivalent for:
*.probe v(0) v(1)
.probe v(?)
***Wildcard equivalent for:
*.print v(n20) v(n21)
.print v(n2?)
***Wildcard equivalent for:
*.probe v(n20, 1) v(n21, 1)
.probe v(n2*, 1)
.end
HSPICE® Simulation and Analysis User Guide
Y-2006.03
247
Chapter 7: Simulation Output
Displaying Simulation Results
Supported Wildcard Templates
v vm vr vi vp vdb vt
i im ir ii ip idb it
p pm pr pi pp pdb pt
lxn<n> lvn<n> (n is a number 0~9)
i1 im1 ir1 ii1 ip1 idb1 it1
i2 im2 ir2 ii2 ip2 idb2 it2
i3 im3 ir3 ii3 ip3 idb3 it3
i4 im4 ir4 ii4 ip4 idb4 it4
iall
For detailed information about the templates, see .PRINT statement (see
Selecting Simulation Output Parameters on page 251).
Using wildcards in statements such as v(n2?) and v(n2*,1) in the
preceding test case (named test wildcard), you can also use the following in
statements (they are not equivalent if you use an .AC statement instead of
a .DC statement):
vm(n2?) vr(n2?) vi(n2?) vp(n2?) vdb(n2?) vt(n2?)
vm(n2*,1) vr(n2*,1) vi(n2*,1) vp(n2*,1) vdb(n2*,1) vt(n2*,1)
Using wildcards in statements such as i(*) in this test wildcard case. You can
also use the following in statements (they are not equivalent if you use an .AC
statement instead of a .DC statement):
im(*) ir(*) ip(*) idb(*) it(*)
iall is an output template for all branch currents of diode, BJT, JFET, or
MOSFET output. For example, iall(m*) is equivalent to:
i1(m*) i2(m*) i3(m*) i4(m*).
Print Control Options
The codes that you can use to specify the element templates for output in
HSPICE or HSPICE RF are:
248
■
.OPTION CO to set column widths in printouts.
■
.WIDTH statement to set the width of a printout.
■
.OPTION INGOLD for output in exponential form.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Displaying Simulation Results
■
.OPTION POST to display high-resolution AvanWaves plots of simulation
results, on either a graphics terminal or a high-resolution laser printer.
■
.OPTION ACCT to generate a detailed accounting report. HSPICE RF does
not support this statement.
Changing the File Descriptor Limit
A simulation that uses a large number of .ALTER statements might fail,
because of the limit on the number of file descriptors. For example, for a Sun
workstation, the default number of file descriptors is 64, so a design with more
than 50 .ALTER statements probably fails, with the following error message:
error could not open output spool file /tmp/tmp.nnn
a critical system resource is inaccessible or exhausted
To prevent this error on a Sun workstation, enter the following operating system
command, before you start the simulation:
limit descriptors 128
For platforms other than Sun workstations, ask your system administrator to
help you increase the number of files that you can open concurrently.
Printing the Subcircuit Output
The following examples demonstrate how to print or plot voltages of nodes that
are in subcircuit definitions, using .PRINT, .PLOT, .PROBE, or .GRAPH.
Note:
In the following example, you can substitute .PROBE, .PLOT, or .GRAPH
instead of .PRINT. HSPICE RF does not support .PLOT or .GRAPH.
Example 1
.GLOBAL vdd vss
X1 1 2 3 nor2
X2 3 4 5 nor2
.SUBCKT nor2 A B Y
.PRINT v(B) v(N1) $ Print statement 1
M1 N1 A vdd vdd pch w=6u l=0.8u
M2 Y B N1 vdd pch w=6u l=0.8u
M3 Y A vss vss vss nch w=3u l=0.8u
M4 Y B vss vss nch w=3u l=0.8u
.ENDS
HSPICE® Simulation and Analysis User Guide
Y-2006.03
249
Chapter 7: Simulation Output
Displaying Simulation Results
Print statement 1 prints out the voltage on the B input node, and on the N1
internal node for every instance of the nor2 subcircuit.
.PRINT v(1) v(X1.A) $ Print statement 2
The preceding .PRINT statement specifies two ways to print the voltage on the
A input of the X1 instance.
.PRINT v(3) v(X1.Y)
v(X2.A) $ Print statement 3
The preceding .PRINT statement specifies three different ways to print the
voltage at the Y output of the X1 instance (or the A input of the X2 instance).
.PRINT v(X2.N1) $ Print statement 4
The preceding .PRINT statement prints the voltage on the N1 internal node of
the X2 instance.
.PRINT i(X1.M1) $ Print statement 5
The preceding .PRINT statement prints out the drain-to-source current,
through the M1 MOSFET in the X1 instance.
Example 2
X1 5 6 YYY
.SUBCKT YYY 15 16
X2 16 36 ZZZ
R1 15 25 1
R2 25 16 1
.ENDS
.SUBCKT ZZZ 16 36
C1 16 0 10P
R3 36 56 10K
C2 56 0 1P
.ENDS
.PRINT V(X1.25) V(X1.X2.56) V(6)
250
Value
Description
V(X1.25)
Local node to the YYY subcircuit definition, which the X1 subcircuit
calls.
V(X1.X2.56)
Local node to the ZZZ subcircuit. The X2 subcircuit calls this node; X1
calls X2.
V(6)
Voltage of node 16, in the X1 instance of the YYY subcircuit.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
This example prints voltage analysis results at node 56, within the X2 and X1
subcircuits. The full path, X1.X2.56, specifies that node 56 is within the X2
subcircuit, which in turn is within the X1 subcircuit.
Selecting Simulation Output Parameters
Parameters provide the appropriate simulation output. To define simulation
parameters, use the .OPTION and .MEASURE statements, and define specific
variable elements.
DC and Transient Output Variables
■
Voltage differences between specified nodes (or between one specified
node and ground).
■
Current output for an independent voltage source.
■
Current output for any element.
■
Current output for a subcircuit pin.
■
Element templates (HSPICE only). For each device type, the templates
contain:
•
values of variables that you set
•
state variables
•
element charges
•
capacitance currents
•
capacitances
•
derivatives
Print Control Options on page 248 summarizes the codes that you can use, to
specify the element templates for output in HSPICE or HSPICE RF.
Nodal Capacitance Output
Syntax
Cap(nxxx)
For nodal capacitance output, HSPICE prints or plots the capacitance of the
specified node nxxxx.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
251
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Example
.print dc Cap(5) Cap(6)
Nodal Voltage
Syntax
V(n1<,n2>)
Parameter
Description
n1, n2
HSPICE or HSPICE RF prints or plots the voltage difference (n1-n2)
between the specified nodes. If you omit n2, HSPICE or HSPICE RF
prints or plots the voltage difference between n1 and ground (node 0).
Current: Independent Voltage Sources
Syntax
I(Vxxx)
Parameter
Description
Vxxx
Voltage source element name. If an independent power supply is
within a subcircuit, then to access its current output, append a dot and
the subcircuit name to the element name. For example, I(X1.Vxxx).
Example
.PLOT TRAN I(VIN)
.PRINT DC I(X1.VSRC)
.PLOT DC I(XSUB.XSUBSUB.VY)
Current: Element Branches
Syntax
In(Wwww)
Iall(Wwww)
252
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Parameter
Description
n
Node position number, in the element statement. For example, if the
element contains four nodes, I3 is the branch current output for the
third node. If you do not specify n, HSPICE or HSPICE RF assumes
the first node.
Wwww
Element name. To access current output for an element in a subcircuit,
append a dot and the subcircuit name to the element name. For
example, I3(X1.Wwww).
Iall (Wwww)
An alias just for diode, BJT, JFET, and MOSFET devices.
■
■
If Wwww is a diode, it is equivalent to:
I1(Wwww) I2(Wwww).
If Wwww is one of the other device types, it is equivalent to:
I1(Wwww) I2(Wwww) I3(Wwww) I4(Wwww)
Example 1
I1(R1)
This example specifies the current through the first R1 resistor node.
Example 2
I4(X1.M1)
This example specifies the current, through the fourth node (the substrate
node) of the M1 MOSFET, defined in the X1 subcircuit.
Example 3
I2(Q1)
The last example specifies the current, through the second node (the base
node) of the Q1 bipolar transistor.
To define each branch circuit, use a single element statement. When HSPICE
or HSPICE RF evaluates branch currents, it inserts a zero-volt power supply, in
series with branch elements.
If HSPICE cannot interpret a .PRINT or .PLOT statement that contains a
branch current, it generates a warning.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
253
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Branch current direction for the elements in Figure 29 through Figure 34 is
defined in terms of arrow notation (current direction), and node position number
(terminal type).
Figure 29
Resistor (node1, node2)
node1
I1 (R1)
R1
node2
I2 (R1)
Figure 30
Inductor (node1, node2); capacitor (node 1, node2)
node1
I1(L1)
I1(C1)
I2(L1)
I2(C1)
node2
Figure 31
254
Diode (node1, node2)
I1 (D1)
node1 (anode, P-type, + node)
I2 (D2)
node2 (anode, N-type, - node)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Figure 32
JFET (node1, node2, node3) - n-channel
node1 (drain node)
I1 (J1)
node2
(gate node)
I2 (J1)
Figure 33
node2 (source node)
I3 (J1)
MOSFET (node1, node2, node3, node4) - n-channel
node1 (drain node)
I1 (M1)
node2 (gate node)
node4 (substrate node)
I4 (M1)
I2 (M1)
node3 (source node)
I3 (M1)
Figure 34
BJT (node1, node2, node3, node4) - npn
node1 (collector node)
I1 (Q1)
node2 (base node)
I2 (Q1)
node4 (substrate node)
I4 (Q1)
node3 (emitter node)
I3 (Q1)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
255
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Current: Subcircuit Pin
Syntax
ISUB(X****.****)
Example
.PROBE ISUB(X1.PIN1)
Power Output
For power calculations, HSPICE or HSPICE RF computes dissipated or stored
power in each passive element (R, L, C), and source (V, I, G, E, F, and H). To
compute this power, HSPICE or HSPICE RF multiplies the voltage across an
element, and its corresponding branch current.
However, for semiconductor devices, HSPICE or HSPICE RF calculates only
the dissipated power. It excludes the power stored in the device junction or
parasitic capacitances, from the device power computation. The following
sections show equations for calculating the power that different types of
devices dissipate.
HSPICE or HSPICE RF also computes the total power dissipated in the circuit,
which is the sum of the power dissipated in:
■
Devices
■
Resistors
■
Independent current sources
■
All dependent sources
For hierarchical designs, HSPICE or HSPICE RF also computes the power
dissipation for each subcircuit.
Note:
For the total power (dissipated power + stored power), HSPICE or HSPICE
RF does not add the power of each independent source (voltage and current
sources).
256
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Print or Plot Power
Note:
To output the instantaneous element power, and the total power dissipation,
use a .PRINT or .PLOT statement in HSPICE.HSPICE RF does not
support .PLOT statements or power variables in DC/transient analysis.
.PRINT <DC | TRAN> P(element_or_subcircuit_name)POWER
HSPICE calculates power only for transient and DC sweep analyses. Use
the .MEASURE statement to compute the average, RMS, minimum, maximum,
and peak-to-peak value of the power. The POWER keyword invokes the total
power dissipation output.
HSPICE RF supports p(instance) but not the POWER variable in DC/transient
analysis.
Example
.PRINT TRAN
P(M1)
P(VIN)
P(CLOAD)
POWER
.PRINT TRAN
P(Q1)
P(DIO)
P(J10)
POWER
.PRINT TRAN
POWER
$ Total transient analysis
* power dissipation
.PLOT DC POWER
P(IIN)
P(RLOAD)
P(R1)
.PLOT DC POWER
P(V1)
P(RLOAD)
P(VS)
.PRINT TRAN P(Xf1) P(Xf1.Xh1)
Diode Power Dissipation
Pd = Vpp' ⋅ ( Ido + Icap ) + Vp'n ⋅ Ido
Parameter
Description
Pd
Power dissipated in the diode.
Ido
DC component of the diode current.
Icap
Capacitive component of the diode current.
Vp'n
Voltage across the junction.
Vpp'
Voltage across the series resistance, RS.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
257
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
BJT Power Dissipation
■
Vertical
Pd = Vc'e' ⋅ Ico + Vb'e' ⋅ Ibo + Vcc' ⋅ Ictot + Vee' ⋅ Ietot + Vsc' ⋅ Iso – Vcc' ⋅Istot
■
Lateral
Pd = Vc'e' ⋅ Ico + Vb'e' ⋅ Ibo + Vcc' ⋅ Ictot + Vbb' ⋅ Ibtot + Vee' ⋅ Ietot
Vsb' ⋅ Iso – Vbb' ⋅Istot
258
Parameter
Description
Ibo
DC component of the base current.
Ico
DC component of the collector current.
Iso
DC component of the substrate current.
Pd
Power dissipated in a BJT.
Ibtot
Total base current (excluding the substrate current).
Ictot
Total collector current (excluding the substrate current).
Ietot
Total emitter current.
Istot
Total substrate current.
Vb'e'
Voltage across the base-emitter junction.
Vbb'
Voltage across the series base resistance, RB.
Vc'e'
Voltage across the collector-emitter terminals.
Vcc'
Voltage across the series collector resistance, RC.
Vee'
Voltage across the series emitter resistance, RE.
Vsb'
Voltage across the substrate-base junction.
Vsc'
Voltage across the substrate-collector junction.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
JFET Power Dissipation
Pd = Vd's' ⋅ Ido + Vgd' ⋅ Igdo + Vgs' ⋅ Igso +
Vs's ⋅ ( Ido + Igso + Icgs ) + Vdd' ⋅ ( Ido – Igdo – Icgd )
Parameter
Description
Icgd
Capacitive component of the gate-drain junction current.
Icgs
Capacitive component of the gate-source junction current.
Ido
DC component of the drain current.
Igdo
DC component of the gate-drain junction current.
Igso
DC component of the gate-source junction current.
Pd
Power dissipated in a JFET.
Vd's'
Voltage across the internal drain-source terminals.
Vdd'
Voltage across the series drain resistance, RD.
Vgd'
Voltage across the gate-drain junction.
Vgs'
Voltage across the gate-source junction.
Vs's
Voltage across the series source resistance, RS.
MOSFET Power Dissipation
Pd = Vd's' ⋅ Ido + Vbd' ⋅ Ibdo + Vbs' ⋅ Ibso +
Vs's ⋅ ( Ido + Ibso + Icbs + Icgs ) + Vdd' ⋅ ( Ido – Ibdo – Icbd – Icgd )
Parameter
Description
Ibdo
DC component of the bulk-drain junction current.
Ibso
DC component of the bulk-source junction current.
Icbd
Capacitive component of the bulk-drain junction current.
Icbs
Capacitive component of the bulk-source junction current.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
259
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Parameter
Description
Icgd
Capacitive component of the gate-drain current.
Icgs
Capacitive component of the gate-source current.
Ido
DC component of the drain current.
Pd
Power dissipated in the MOSFET.
Vbd'
Voltage across the bulk-drain junction.
Vbs'
Voltage across the bulk-source junction.
Vd's'
Voltage across the internal drain-source terminals.
Vdd'
Voltage across the series drain resistance, RD.
Vs's
Voltage across the series source resistance, RS.
AC Analysis Output Variables
Output variables for AC analysis include:
■
Voltage differences between specified nodes (or between one specified
node and ground).
■
Current output for an independent voltage source.
■
Current output for a subcircuit pin.
■
Element branch current.
■
Impedance (Z), admittance (Y), hybrid (H), and scattering (S) parameters.
■
Input and output impedance, and admittance.
Table 24 lists AC output variable types. In this table, the type symbol is
appended to the variable symbol, to form the output variable name. For
example, VI is the imaginary part of the voltage, or IM is the magnitude of the
current.
260
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Table 24
AC Output Variable Types
Type Symbol
Variable Type
DB
decibel
I
imaginary part
M
magnitude
P
phase
R
real part
T
group delay
Specify real or imaginary parts, magnitude, phase, decibels, and group delay
for voltages and currents.
Nodal Capacitance Output
Syntax
Cap(nxxx)
For nodal capacitance output, HSPICE prints or plots the capacitance of the
specified node nxxxx.
Example
.print ac Cap(5) Cap(6)
Nodal Voltage
Syntax
Vz(n1<,n2>)
Parameter
Description
z
Specifies the voltage output type (see Table 24 on page 261)
n1, n2
Specifies node names. If you omit n2, HSPICE or HSPICE RF
assumes ground (node 0).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
261
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Example
This example applies to HSPICE, but not HSPICE RF. It plots the magnitude of
the AC voltage of node 5, using the VM output variable. HSPICE uses the VDB
output variable to plot the voltage at node 5, and uses the VP output variable to
plot the phase of the nodal voltage at node 5.
.PLOT AC VM(5) VDB(5) VP(5)
HSPICE and SPICE Methods for Producing Complex Results
To produce complex results, an AC analysis uses either the SPICE or HSPICE
method, and the .OPTION ACOUT control option, to calculate the values of real
or imaginary parts for complex voltages of AC analysis, and their magnitude,
phase, decibel, and group delay values. The default for HSPICE is ACOUT=1.
To use the SPICE method, set ACOUT=0.
A typical use of the SPICE method is to calculate the nodal vector difference,
when comparing adjacent nodes in a circuit. You can use this method to find
the phase or magnitude across a capacitor, inductor, or semiconductor device.
Use the HSPICE method to calculate an inter-stage gain in a circuit (such as an
amplifier circuit), and to compare its gain, phase, and magnitude.
The following examples define the AC analysis output variables for the HSPICE
method, and then for the SPICE method.
HSPICE Method Example:
Real and imaginary:
VR(N1,N2)= REAL [V(N1,0)] - REAL [V(N2,0)]
VI(N1,N2)= IMAG [V(N1,0)] - IMAG [V(N2,0)]
Magnitude:
VM(N1,0)= [VR(N1,0)2 + VI(N1,0)2]0.5
VM(N2,0)= [VR(N2,0)2 + VI(N2,0)2]0.5
VM(N1,N2)= VM(N1,0) - VM(N2,0)
Phase:
VP(N1,0)= ARCTAN[VI(N1,0)/VR(N1,0)]
VP(N2,0)= ARCTAN[VI(N2,0)/VR(N2,0)]
VP(N1,N2)= VP(N1,0) - VP(N2,0)
Decibel:
VDB(N1,0)=20 ⋅ LOG10[VM(N1,0)]
VDB(N1,N2)= 20 ⋅ LOG10(VM(N1,0)/VM(N2,0))
262
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Parameter
Description
n
Node position number, in the element statement. For example, if the
element contains four nodes, IM3 denotes the magnitude of the
branch current output for the third node.
Wwww
Element name. If the element is within a subcircuit, then to access its
current output, append a dot and the subcircuit name to the element
name. For example, IM3(X1.Wwww).
.PRINT AC IP1(Q5) IM1(Q5) IDB4(X1.M1)
If you use the form In(Xxxx) for AC analysis output, then HSPICE or HSPICE
RF prints the magnitude value, IMn(Xxxx).
Current: Subcircuit Pin
Syntax
ISUB(X****.****)
Example
.PROBE ISUB(X1.PIN1)
Group Time Delay
The TD group time delay is associated with AC analysis. TD is the negative
derivative of the phase in radians, with respect to radian frequency. HSPICE or
HSPICE RF uses the difference method to compute TD:
phase2 – phase1 )1 - ⋅ (----------------------------------------------TD = – -------( f2 – f1 )
360
phase1 and phase2 are the phases (in degrees) of the specified signal, at the
f1 and f2 frequencies (in hertz).
Syntax
.PRINT AC VT(10) VT(2,25) IT(RL)
.PLOT AC IT1(Q1) IT3(M15) IT(D1)
Note:
Because the phase has a discontinuity every 360×, TD shows the same
discontinuity, even though TD is continuous. The .PRINT example applies
to both HSPICE and HSPICE RF, but the .PLOT example applies only to
HSPICE.
264
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Example
INTEG.SP ACTIVE INTEGRATOR
****** INPUT LISTING
******
V1
1
0
.5
AC
1
R1
1
2
2K
C1
2
3
5NF
E3
3
0
2 0 -1000.0
.AC DEC
15
1K
100K
.PLOT AC
VT(3)
(0,4U)
.END
VP(3)
Network
Syntax
Xij (z), ZIN(z), ZOUT(z), YIN(z), YOUT(z)
Parameter
Description
X
Specifies Z (impedance), Y (admittance), H (hybrid), or S (scattering).
ij
i and j can be 1 or 2. They identify the matrix parameter to print.
z
Output type (see Table 24 on page 261). If you omit z, HSPICE or
HSPICE RF prints the magnitude of the output variable.
ZIN
Input impedance. For a one-port network, ZIN, Z11, and H11 are the
same.
ZOUT
Output impedance.
YIN
Input admittance. For a one-port network, YIN and Y11 are the same.
YOUT
Output admittance.
Example
.PRINT
.PRINT
.PLOT
AC
AC
AC
Z11(R)
ZIN(R)
S22(M)
Z12(R)
ZIN(I)
S22(P)
Y21(I)
Y22
S11
S11(DB)
YOUT(M)
YOUT(P)
H11(M)
S21(R)
H21(P)
H12(R)
The .PRINT examples apply to both HSPICE and HSPICE RF. The .PLOT
example applies only to HSPICE.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
265
Chapter 7: Simulation Output
Selecting Simulation Output Parameters
Noise and Distortion
This section describes the variables used for noise and distortion analysis.
Syntax
ovar <(z)>
Parameter
Description
ovar
Noise and distortion analysis parameter. It can be ONOISE (output
noise), INOISE (equivalent input noise), or any of the distortion
analysis parameters (HD2, HD3, SIM2, DIM2, DIM3).
z
Output type (only for distortion). If you omit z, HSPICE or HSPICE RF
outputs the magnitude of the output variable.
Example
.PRINT DISTO HD2(M) HD2(DB)
Prints the magnitude and decibel values of the second harmonic distortion
component, through the load resistor that you specified in the .DISTO
statement (not shown). You cannot use the .DISTO statement in HSPICE RF.
.PLOT NOISE INOISE ONOISE
Note:
You can specify the noise and distortion output variable, and other AC output
variables, in the .PRINT AC or .PLOT AC statements. The .PRINT
example applies to both HSPICE and HSPICE RF. The .PLOT example
applies only to HSPICE.
Element Template Output
(HSPICE) The .PRINT, .PROBE, .PLOT, and .GRAPH statements use
element templates to output user-input parameters, state variables, stored
charges, capacitor currents, capacitances, and derivatives of variables.
Element templates are listed at the end of this chapter.t
266
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
Syntax
Elname:Property
Parameter
Description
Elname
Name of the element.
Property
Property name of an element, such as a user-input parameter, state
variable, stored charge, capacitance current, capacitance, or
derivative of a variable.
The alias is:
LVnn(Elname)
LXnn(Elname)
Parameter
Description
LV
Form to obtain output of user-input parameters, and state variables.
LX
Form to obtain output of stored charges, capacitor currents,
capacitances, and derivatives of variables.
nn
Code number for the desired parameter (listed in tables in this
section).
Elname
Name of the element.
Example
.PLOT TRAN V(1,12) I(X2.VSIN) I2(Q3) DI01:GD
.PRINT TRAN X2.M1:CGGBO M1:CGDBO X2.M1:CGSBO
The .PRINT example applies to both HSPICE and HSPICE RF; the .PLOT
example applies to HSPICE only.
Specifying User-Defined Analysis (.MEASURE)
Use the .MEASURE statement to modify information, and to define the results of
successive HSPICE or HSPICE RF simulations.
Computing the measurement results is based on postprocessing output. If you
use the INTERP option to reduce the size of the postprocessing output, then
the measurement results can contain interpolation errors. For more
HSPICE® Simulation and Analysis User Guide
Y-2006.03
267
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
information, see the .OPTION INTERP option in the HSPICE Command
Reference.
Fundamental measurement modes in HSPICE are:
■
Rise, fall, and delay
■
Find-when
■
Equation evaluation
■
Average, RMS, min, max, and peak-to-peak
■
Integral evaluation
■
Derivative evaluation
■
Relative error
If a .MEASURE statement does not execute, then HSPICE or HSPICE RF
writes 0.0e0 in the .mt# file as the .MEASURE result, and writes FAILED in the
output listing file. Use .OPTION MEASFAIL to write results to the .mt#, .ms#,
or .ma# files. For more information, see the .OPTION MEASFAIL option in the
HSPICE Command Reference.
Note:
Beginning with the 2004.03 release, the .mt# format consists of 72
characters in a line and fields that contain 16 characters each. The extra line
that existed in previous releases has been removed.
To control the output variables, listed in .MEASURE statements, use
the .PUTMEAS option. For more information, see the .OPTION PUTMEAS
option in the HSPICE Command Reference
In versions of HSPICE before 2003.09, to automatically sort large numbers
of .MEASURE statements, you could use the MEASSORT option. Starting in
version 2003.09, this option is obsolete. Now the measure performance is
order-independent, and HSPICE ignores this option.
.MEASURE Statement Order
The .MEASURE statement matches the last analysis command in the netlist
before the .MEASURE statement.
Example
.tran 20p 1.0n sweep sigma -3 3 0.5
.tran 20p 1.0n sweep monte=20
.meas mover max v(2,1)
268
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
In this example, .meas matches the second .tran statement and generates
only one measure output file.
.MEASURE Parameter Types
You cannot use measurement parameter results that the .PARAM statements
in .SUBCKT blocks produce, outside of the subcircuit. That is, you cannot pass
any measurement parameters defined in .SUBCKT statements, as bottom-up
parameters in hierarchical designs.
Measurement parameter names must not conflict with standard parameter
names. HSPICE or HSPICE RF issues an error message, if it encounters a
measurement parameter with the same name as a standard parameter
definition.
To prevent .MEASURE statement parameters from overwriting parameter values
in other statements, HSPICE or HSPICE RF keeps track of parameter types. If
you use the same parameter name in both a .MEASURE statement and
a .PARAM statement at the same hierarchical level, simulation terminates and
reports an error.
No error occurs if parameter assignments are at different hierarchical
levels. .PRINT statements that occur at different levels, do not print
hierarchical information for parameter name headings.
Example
In HSPICE RF simulation output, you cannot apply .MEASURE to waveforms
generated from another .MEASURE statement in a parameter sweep.
The following example illustrates how HSPICE or HSPICE RF handles
.MEASURE statement parameters.
...
.MEASURE tran length TRIG v(clk) VAL=1.4
+ TD=11ns RISE=1 TARGv(neq) VAL=1.4 TD=11ns
+ RISE=1
.SUBCKT path out in width=0.9u length=600u
+ rm1 in m1 m2mg w='width' l='length/6'
...
.ENDS
In the above listing, the length in the resistor statement:
rm1 in m1 m2mg w='width' l='length/6'
does not inherit its value from length in the .MEASURE statement:
HSPICE® Simulation and Analysis User Guide
Y-2006.03
269
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
.MEASURE tran length ...
because they are of different types.
The correct value of l in rm1 should be:
l=length/6=100u
The value should not be derived from a measured value in transient analysis.
FIND and WHEN Functions
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.
You can use these measure statements in unity gain frequency or phase
measurements. You can also use these statements to measure the time,
frequency, or any parameter value:
■
When two signals cross each other.
■
When a signal crosses a constant value.
The measurement starts after a specified time delay, TD. To find a specific
event, set RISE, FALL, or CROSS to a value (or parameter), or specify LAST for
the last event.
LAST is a reserved word; you cannot use it as a parameter name in the above
measure statements. For definitions of parameters of the measure statement,
see Displaying Simulation Results on page 243.
Equation Evaluation
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. If equation or expression includes node
voltages or branch currents, Unexpected results may incur.
270
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
Average, RMS, MIN, MAX, INTEG, and PP
Average (AVG), RMS, MIN, MAX, and peak-to-peak (PP) measurement modes
report statistical functions of the output variable, rather than analysis values.
■
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.
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.
INTEGRAL Function
The INTEGRAL function reports the integral of an output variable, over a
specified period.
DERIVATIVE Function
The DERIVATIVE function provides the derivative of:
■
An output variable, at a specified time or frequency.
■
Any sweep variable, depending on the type of analysis.
■
A specified output variable, when some specific event occurs.
In the HSPICE RF example below, the SLEW measurement provides the slope
of V(OUT) during the first time, when V(1) is 90% of VDD.
.MEAS TRAN SLEW DERIV V(OUT) WHEN V(1)=‘0.90*VDD’
HSPICE® Simulation and Analysis User Guide
Y-2006.03
271
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
ERROR Function
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 function. With this
format, you can specify a group of parameters to vary, to match the calculated
value and the measured data.
Error Equations
ERR
1. ERR sums the squares of (M-C)/max (M, MINVAL) for each point.
2. It then divides by the number of points.
3. Finally, it calculates the square root of the result.
•
M (meas_var) is the measured value of the device or circuit response.
•
C (calc_var) is the calculated value of the device or circuit response.
•
NPTS is the number of data points.
NPTS
1
ERR = --------------- ⋅
NPTS
∑
i=1
1/2
2
Mi – Ci
⎛ ---------------------------------------------⎞
⎝ max (MINVAL,M i)⎠
ERR1
ERR1 computes the relative error at each point. For NPTS points, HSPICE or
HSPICE RF calculates NPTS ERR1 error functions. For device
characterization, the ERR1 approach is more efficient than the other error
functions (ERR, ERR2, ERR3).
Mi – Ci
- , i=1,NPTS
ERR1 i = --------------------------------------------max (MINVAL,M i)
272
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Specifying User-Defined Analysis (.MEASURE)
HSPICE or HSPICE RF does not print out each calculated ERR1 value. When
you set the ERR1 option, HSPICE or HSPICE RF calculates an ERR value, as
follows:
1/2
NPTS
1
ERR = --------------- ⋅
NPTS
∑
ERR1 i2
i=1
ERR2
This option computes the absolute relative error, at each point. For NPTS
points, HSPICE or HSPICE RF calls NPTS error functions.
Mi – Ci
ERR2 i = --------------------------------------------- , i=1,NPTS
max (MINVAL,M i)
The returned value printed for ERR2 is:
NPTS
1
ERR = --------------- ⋅
NPTS
∑
ERR2 i
i=1
ERR3
M
± log ------i
Ci
ERR3 i = ---------------------------------------------------------------- , i=1,NPTS
log [ max (MINVAL, M i ) ]
The + and - signs correspond to a positive and negative M/C ratio.
Note:
If the M measured value is less than MINVAL, HSPICE or HSPICE RF uses
MINVAL instead. If the absolute value of M is less than the IGNOR or YMIN
value, or greater than the YMAX value, the error calculation does not
consider this point.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
273
Chapter 7: Simulation Output
Reusing Simulation Output as Input Stimuli
Reusing Simulation Output as Input Stimuli
You can use the .STIM statement to reuse the results (output) of one
simulation, as input stimuli in a new simulation.
Note:
.STIM is an abbreviation of .STIMULI. You can use either form to specify
this statement in HSPICE. HSPICE RF does not support this statement.
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.
For the syntax and description of the .STIM statement, see the .STIM
command in the HSPICE Command Reference.
Output Files
The .STIM statement generates the following output files:
274
Output File Type
Extension
PWL Source
.pwl$_tr#The .STIM statement writes PWL source results to
output_file.pwl$_tr#. This output file results from a .STIM <tran>
pwl statement in the input file.
Data Card
.dat$_tr#, .dat$_ac#, or .dat$_sw#The .STIM
statement writes DATA Card results to output_file.dat$_sw#,
output_file.dat$_ac#, or output_file.dat$_tr#. This output file is
the result of a .stim <tran| ac|dc> data statement in the input file.
Digital Vector File
.vec$_tr#The .STIM statement writes Digital Vector File
results to output_file.vec$_tr#. This output file is the result of
a .stim <tran> vec statement in the input file.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Element Template Listings
Symbol
Description
tr | ac | sw
■
■
■
tr=transient analysis.
ac=AC analysis.
sw=DC sweep analysis.
#
Either a sweep number, or a hard-copy file number. For a single
sweep run, the default number is 0.
$
Serial number of the current .STIM statement, within statements of
the same stimulus type (pwl, data, or vec).
$=0 ~ n-1 (n is the number of the .STIM statement of that type). The
initial $ value is 0.
For example, if you specify three .STIM pwl statements, HSPICE
generates three PWL output files, with the suffix names pwl0_tr#,
pwl1_tr#, and pwl2_tr#.
Element Template Listings
This section applies only to HSPICE. HSPICE RF does not support element
template output.
Table 25
Resistor (R Element)
Name
Alias
Description
G
LV1
Conductance at analysis temperature.
R
LV2
Resistance at analysis temperature.
TC1
LV3
First temperature coefficient.
TC2
LV4
Second temperature coefficient.
Table 26
Capacitor (C Element)
Name
Alias
Description
CEFF
LV1
Computed effective capacitance.
IC
LV2
Initial condition.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
275
Chapter 7: Simulation Output
Element Template Listings
Table 26
Name
Alias
Description
Q
LX0
Charge, stored in capacitor.
CURR
LX1
Current, flowing through capacitor.
VOLT
LX2
Voltage, across capacitor.
–
LX3
Capacitance (not used after HSPICE releases after 95.3).
Table 27
Inductor (L Element)
Name
Alias
Description
LEFF
LV1
Computed effective inductance.
IC
LV2
Initial condition.
FLUX
LX0
Flux, in the inductor.
VOLT
LX1
Voltage, across inductor.
CURR
LX2
Current, flowing through inductor.
–
LX4
Inductance (not used after HSPICE releases after 95.3).
Table 28
Mutual Inductor (K Element)
Name
Alias
Description
K
LV1
Mutual inductance.
Table 29
276
Capacitor (C Element) (Continued)
Voltage-Controlled Current Source (G Element)
Name
Alias
Description
CURR
LX0
Current, through the source, if VCCS.
R
LX0
Resistance value, if VCR.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Element Template Listings
Table 29
Voltage-Controlled Current Source (G Element) (Continued)
Name
Alias
Description
C
LX0
Capacitance value, if VCCAP.
CV
LX1
Controlling voltage.
CQ
LX1
Capacitance charge, if VCCAP.
DI
LX2
Derivative of the source current, relative to the control
voltage.
ICAP
LX2
Capacitance current, if VCCAP.
VCAP
LX3
Voltage, across capacitance, if VCCAP.
Table 30
Voltage-Controlled Voltage Source (E Element)
Name
Alias
Description
VOLT
LX0
Source voltage.
CURR
LX1
Current, through source.
CV
LX2
Controlling voltage.
DV
LX3
Derivative of the source voltage, relative to the control
current.
Table 31
Current-Controlled Current Source (F Element)
Name
Alias
Description
CURR
LX0
Current, through source.
CI
LX1
Controlling current.
DI
LX2
Derivative of the source current, relative to the control
current.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
277
Chapter 7: Simulation Output
Element Template Listings
Table 32
Name
Alias
Description
VOLT
LX0
Source voltage.
CURR
LX1
Source current.
CI
LX2
Controlling current.
DV
LX3
Derivative of the source voltage, relative to the control
current.
Table 33
Independent Voltage Source (V Element)
Name
Alias
Description
VOLT
LV1
DC/transient voltage.
VOLTM
LV2
AC voltage magnitude.
VOLTP
LV3
AC voltage phase.
Table 34
Independent Current Source (I Element)
Name
Alias
Description
CURR
LV1
DC/transient current.
CURRM
LV2
AC current magnitude.
CURRP
LV3
AC current phase.
Table 35
278
Current-Controlled Voltage Source (H Element)
Diode (D Element)
Name
Alias
Description
AREA
LV1
Diode area factor.
AREAX
LV23
Area, after scaling.
IC
LV2
Initial voltage, across diode.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Element Template Listings
Table 35
Diode (D Element) (Continued)
Name
Alias
Description
VD
LX0
Voltage, across diode (VD), excluding RS (series
resistance).
IDC
LX1
DC current, through diode (ID), excluding RS. Total diode
current is the sum of IDC and ICAP.
GD
LX2
Equivalent conductance (GD).
QD
LX3
Charge of diode capacitor (QD).
ICAP
LX4
Current, through the diode capacitor.
Total diode current is the sum of IDC and ICAP.
C
LX5
Total diode capacitance.
PID
LX7
Photo current, in diode.
Table 36
BJT (Q Element)
Name
Alias
Description
AREA
LV1
Area factor.
ICVBE
LV2
Initial condition for base-emitter voltage (VBE).
ICVCE
LV3
Initial condition for collector-emitter voltage (VCE).
MULT
LV4
Number of multiple BJTs.
FT
LV5
FT (Unity gain bandwidth).
ISUB
LV6
Substrate current.
GSUB
LV7
Substrate conductance.
LOGIC
LV8
LOG 10 (IC).
LOGIB
LV9
LOG 10 (IB).
BETA
LV10
BETA.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
279
Chapter 7: Simulation Output
Element Template Listings
Table 36
280
BJT (Q Element) (Continued)
Name
Alias
Description
LOGBETAI
LV11
LOG 10 (BETA) current.
ICTOL
LV12
Collector current tolerance.
IBTOL
LV13
Base current tolerance.
RB
LV14
Base resistance.
GRE
LV15
Emitter conductance, 1/RE.
GRC
LV16
Collector conductance, 1/RC.
PIBC
LV18
Photo current, base-collector.
PIBE
LV19
Photo current, base-emitter.
VBE
LX0
VBE.
VBC
LX1
Base-collector voltage (VBC).
CCO
LX2
Collector current (CCO).
CBO
LX3
Base current (CBO).
GPI
LX4
gπ=¹ib /¹vbe, constant vbc.
GU
LX5
gμ=¹ib /¹vbc, constant vbe.
GM
LX6
gm=¹ic /¹vbe+ ¹ic /¹vbe, constant vce.
G0
LX7
g0=¹ic /¹vce, constant vbe.
QBE
LX8
Base-emitter charge (QBE).
CQBE
LX9
Base-emitter charge current (CQBE).
QBC
LX10
Base-collector charge (QBC).
CQBC
LX11
Base-collector charge current (CQBC).
QCS
LX12
Current-substrate charge (QCS).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Element Template Listings
Table 36
BJT (Q Element) (Continued)
Name
Alias
Description
CQCS
LX13
Current-substrate charge current (CQCS).
QBX
LX14
Base-internal base charge (QBX).
CQBX
LX15
Base-internal base charge current (CQBX).
GXO
LX16
1/Rbeff Internal conductance (GXO).
CEXBC
LX17
Base-collector equivalent current (CEXBC).
–
LX18
Base-collector conductance (GEQCBO), (not used in
HSPICE releases after 95.3).
CAP_BE
LX19
cbe capacitance (Cπ).
CAP_IBC
LX20
cbc internal base-collector capacitance (Cμ).
CAP_SCB
LX21
csc substrate-collector capacitance for vertical transistors.
csb substrate-base capacitance for lateral transistors.
CAP_XBC
LX22
cbcx external base-collector capacitance.
CMCMO
LX23
¹(TF*IBE) /¹vbc.
VSUB
LX24
Substrate voltage.
Table 37
JFET (J Element)
Name
Alias
Description
AREA
LV1
JFET area factor.
VDS
LV2
Initial condition for drain-source voltage.
VGS
LV3
Initial condition for gate-source voltage.
PIGD
LV16
Photo current, gate-drain in JFET.
PIGS
LV17
Photo current, gate-source in JFET.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
281
Chapter 7: Simulation Output
Element Template Listings
Table 37
282
JFET (J Element) (Continued)
Name
Alias
Description
VGS
LX0
VGS.
VGD
LX1
Gate-drain voltage (VGD).
CGSO
LX2
Gate-to-source (CGSO).
CDO
LX3
Drain current (CDO).
CGDO
LX4
Gate-to-drain current (CGDO).
GMO
LX5
Transconductance (GMO).
GDSO
LX6
Drain-source transconductance (GDSO).
GGSO
LX7
Gate-source transconductance (GGSO).
GGDO
LX8
Gate-drain transconductance (GGDO).
QGS
LX9
Gate-source charge (QGS).
CQGS
LX10
Gate-source charge current (CQGS).
QGD
LX11
Gate-drain charge (QGD).
CQGD
LX12
Gate-drain charge current (CQGD).
CAP_GS
LX13
Gate-source capacitance.
CAP_GD
LX14
Gate-drain capacitance.
–
LX15
Body-source voltage (not used after HSPICE release 95.3).
QDS
LX16
Drain-source charge (QDS).
CQDS
LX17
Drain-source charge current (CQDS).
GMBS
LX18
Drain-body (backgate) transconductance (GMBS).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Element Template Listings
Table 38
MOSFET
Name
Alias
Description
L
LV1
Channel length (L).
W
LV2
Channel width (W).
AD
LV3
Area of the drain diode (AD).
AS
LV4
Area of the source diode (AS).
ICVDS
LV5
Initial condition for drain-source voltage (VDS).
ICVGS
LV6
Initial condition for gate-source voltage (VGS).
ICVBS
LV7
Initial condition for bulk-source voltage (VBS).
–
LV8
Device polarity:
■
■
1=forward
-1=reverse (not used after HSPICE releases after 95.3).
VTH
LV9
Threshold voltage (bias dependent).
VDSAT
LV10
Saturation voltage (VDSAT).
PD
LV11
Drain diode periphery (PD).
PS
LV12
Source diode periphery (PS).
RDS
LV13
Drain resistance (squares), (RDS).
RSS
LV14
Source resistance (squares), (RSS).
XQC
LV15
Charge-sharing coefficient (XQC).
GDEFF
LV16
Effective drain conductance (1/RDeff).
GSEFF
LV17
Effective source conductance (1/RSeff).
CDSAT
LV18
Drain-bulk saturation current, at -1 volt bias.
CSSAT
LV19
Source-bulk saturation current, at -1 volt bias.
VDBEFF
LV20
Effective drain bulk voltage.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
283
Chapter 7: Simulation Output
Element Template Listings
Table 38
284
MOSFET (Continued)
Name
Alias
Description
BETAEFF
LV21
BETA, effective.
GAMMAEFF
LV22
GAMMA, effective.
DELTAL
LV23
ΔL (MOS6 amount of channel length modulation), (valid only
for LEVELs 1, 2, 3 and 6).
UBEFF
LV24
UB effective (valid only for LEVELs 1, 2, 3 and 6).
VG
LV25
VG drive (valid only for LEVELs 1, 2, 3 and 6).
VFBEFF
LV26
VFB effective.
–
LV31
Drain current tolerance (not used in HSPICE releases after
95.3).
IDSTOL
LV32
Source-diode current tolerance.
IDDTOL
LV33
Drain-diode current tolerance.
COVLGS
LV36
Gate-source overlap capacitance.
COVLGD
LV37
Gate-drain overlap capacitance.
COVLGB
LV38
Gate-bulk overlap capacitance.
VBS
LX1
Bulk-source voltage (VBS).
VGS
LX2
Gate-source voltage (VGS).
VDS
LX3
Drain-source voltage (VDS).
CDO
LX4
DC-drain current (CDO).
CBSO
LX5
DC source-bulk diode current (CBSO).
CBDO
LX6
DC drain-bulk diode current (CBDO).
GMO
LX7
DC-gate transconductance (GMO).
GDSO
LX8
DC drain-source conductance (GDSO).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 7: Simulation Output
Element Template Listings
Table 38
MOSFET (Continued)
Name
Alias
Description
GMBSO
LX9
DC-substrate transconductance (GMBSO).
GBDO
LX10
Conductance of the drain diode (GBDO).
GBSO
LX11
Conductance of the source diode (GBSO).
Meyer and Charge Conservation Model Parameters
QB
LX12
Bulk charge (QB).
CQB
LX13
Bulk-charge current (CQB).
QG
LX14
Gate charge (QG).
CQG
LX15
Gate-charge current (CQG).
QD
LX16
Channel charge (QD).
CQD
LX17
Channel-charge current (CQD).
CGGBO
LX18
CGGBO = ∂Qg/ ∂Vgb =CGS + CGD + CGB
CGDBO
LX19
CGDBO = ∂Qg/ ∂Vdb , (for Meyer CGD=-CGDBO)
CGSBO
LX20
CGSBO = ∂Qg/ ∂Vsb , (for Meyer CGS=-CGSBO)
CBGBO
LX21
CBGBO = ∂Qb/ ∂Vgb , (for Meyer CGB=-CBGBO)
CBDBO
LX22
CBDBO = ∂Qb/ ∂Vdb
CBSBO
LX23
CBSBO = ∂Qb/ ∂Vsb
QBD
LX24
Drain-bulk charge (QBD).
–
LX25
Drain-bulk charge current (CQBD), (not used in HSPICE
releases after 95.3).
QBS
LX26
Source-bulk charge (QBS).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
285
Chapter 7: Simulation Output
Element Template Listings
Table 38
Name
Alias
Description
–
LX27
Source-bulk charge current (CQBS), (not used after
HSPICE releases after 95.3).
CAP_BS
LX28
Bulk-source capacitance.
CAP_BD
LX29
Bulk-drain capacitance.
CQS
LX31
Channel-charge current (CQS).
CDGBO
LX32
CDGBO = ∂Qd/ ∂Vgb
CDDBO
LX33
CDDBO = ∂Qd/ ∂Vdb
CDSBO
LX34
CDSBO = ∂Qd/ ∂Vsb
Table 39
Saturable Core Element (K Element)
Name
Alias
Description
MU
LX0
Dynamic permeability (mu), Weber/(amp-turn-meter).
H
LX1
Magnetizing force (H), Ampere-turns/meter.
B
LX2
Magnetic flux density (B), Webers/meter2.
Table 40
286
MOSFET (Continued)
Saturable Core Winding
Name
Alias
Description
LEFF
LV1
Effective winding inductance (Henry).
IC
LV2
Initial condition.
FLUX
LX0
Flux, through winding (Weber-turn).
VOLT
LX1
Voltage, across winding (Volt).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
8
Initializing DC/Operating Point Analysis
8
Describes DC initialization and operating point analysis.
For descriptions of individual HSPICE commands referenced in this chapter,
see the HSPICE Command Reference.
Simulation Flow
Figure 35 shows the simulation flow for DC analysis in Synopsys HSPICE and
HSPICE RF.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
287
Chapter 8: Initializing DC/Operating Point Analysis
Initialization and Analysis
Figure 35
DC Initialization and Operating Point Analysis Simulation Flow
Simulation Experiment
Transient
DC
Operating point
Sweep analysis
simulation
AC
DC-related AC
small-signal analysis
.DCMATCH
.PZ
.OPTION: Tolerance
ABSI (ABSTOL)
ABSMOS
ABSV
ABSVDC
KCLTEST
RELI
RELMOS
RELV
RELVDC
Matrix
ITL1
NOPIV
PIVOT
PIVREF
PIVREL
PIVTOL
SPARSE
NOTOP
Monte Carlo
analysis
.SENS
.TF
Convergence
CONVERGE
CSHDC
DCFOR
DCHOLD
DCON
DCSTEP
DCTRAN
DV
GMAX
GMINDC
GRAMP
GSHUNT
ICSWEEP
NEWTOL
OFF
Limit
RESMIN
Initialization and Analysis
Before it performs .OP, .DC sweep, .AC, or .TRAN analyses, HSPICE or
HSPICE RF first sets the DC operating point values for all nodes and sources.
To do this, HSPICE or HSPICE RF does one of the following:
■
Calculates all values
■
Applies values specified in .NODESET and .IC statements
■
Applies values stored in an initial conditions file.
The .OPTION OFF statement, and the OFF and IC=val element parameters,
also control initialization.
288
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Initialization and Analysis
Initialization is fundamental to simulation. HSPICE or HSPICE RF starts any
analysis with known nodal voltages (or initial estimates for unknown voltages)
and some branch currents. It then iteratively finds the exact solution. Initial
estimates that are close to the exact solution increase the likelihood of a
convergent solution and a lower simulation time.
A transient analysis first calculates a DC operating point using the DC
equivalent model of the circuit (unless you specify the UIC parameter in
the .TRAN statement). HSPICE or HSPICE RF then uses the resulting DC
operating point as an initial estimate to solve the next timepoint in the transient
analysis.
Here’s how this is done:
1. If you do not provide an initial guess or if you provide only partial information,
HSPICE or HSPICE RF provides a default estimate for each node in the
circuit.
2. HSPICE or HSPICE RF then uses this estimate to iteratively find the exact
solution.
The .NODESET and statements supply an initial guess for the exact DC
solution of nodes within a circuit.
3. To set any circuit node to any value, use the .NODESET statement.
4. HSPICE or HSPICE RF then connects a voltage source equivalent, to each
initialized node (a current source, with a GMAX parallel conductance, set with
a .OPTION statement).
5. HSPICE or HSPICE RF next calculates a DC operating point, with
the .NODESET voltage source equivalent connected.
6. HSPICE or HSPICE RF disconnects the equivalent voltage sources, which
you set in the .NODESET statement, and recalculates the DC operating
point.
This is the DC operating point solution.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
289
Chapter 8: Initializing DC/Operating Point Analysis
Initialization and Analysis
Figure 36
Equivalent Voltage Source: NODESET and .IC
I=GMAX*V
GMAX
To Initialization
Node
The .IC statement provides both an initial guess and a solution for selected
nodes within the circuit. Nodes that you initialize with the .IC statement
become part of the solution of the DC operating point.
You can also use the OFF option to initialize active devices. The OFF option
works with .IC and .NODESET voltages as follows:
1. If the netlist includes any .IC or .NODESET statements, HSPICE or
HSPICE RF sets node voltages, according to those statements.
2. If you set the OFF option, then HSPICE or HSPICE RF sets values to zero
for the terminal voltages of all active devices (BJTs, diodes, MOSFETs,
JFETs, MESFETs) that are not set in .IC or .NODESET statements, or by
sources.
3. If element statements specify any IC parameters, HSPICE or HSPICE RF
sets those initial conditions.
4. HSPICE or HSPICE RF uses the resulting voltage settings, as the initial
guess at the operating point.
Use OFF to find an exact solution, during an operating point analysis, in a
large circuit. The majority of device terminals are at zero volts for the
operating point solution. To initialize the terminal voltages to zero for
selected active devices, set the OFF parameter in the element statements
for those devices.
After HSPICE finds a DC operating point, use .SAVE to store operatingpoint node voltages in a <design>.ic file. Then use the .LOAD statement to
restore operating-point values, from the ic file for later analyses.
Note:
HSPICE RF does not support the .SAVE and .LOAD (save and restart)
statements.
290
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
DC Initialization and Operating Point Calculation
When you set initial conditions for Transient Analysis:
■
If you include UIC in a .TRAN statement, HSPICE or HSPICE RF starts a
transient analysis, using node voltages specified in an .IC statement.
■
Use the .OP statement, to store an estimate of the DC operating point,
during a transient analysis.
■
HSPICE RF does not output node voltage from operating point (.OP), if time
(t) < 0.
■
An internal timestep too small error message indicates that the circuit failed
to converge. The cause of the failure can be that HSPICE or HSPICE RF
cannot use stated initial conditions to calculate the actual DC operating
point.
DC Initialization and Operating Point Calculation
You use a .OP statement in HSPICE or HSPICE RF to:
■
Calculate the DC operating point of a circuit
■
Produce an operating point during a transient analysis
A simulation can only have one .OP statement.
.OP Statement — Operating Point
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 keyword in
a .TRAN analysis statement, then simulation omits the time=0 operating point
analysis, and issues a warning in the output listing.
Output
***** OPERATING POINT INFORMATION TNOM=25.000 TEMP=25.000
***** OPERATING POINT STATUS IS ALL SIMULATION TIME IS 0.
NODE
VOLTAGE NODE
VOLTAGE NODE
VOLTAGE
+ 0:2=0 0:3=437.3258M 0:4=455.1343M
HSPICE® Simulation and Analysis User Guide
Y-2006.03
291
Chapter 8: Initializing DC/Operating Point Analysis
DC Initialization and Operating Point Calculation
+ 0:5=478.6763M 0:6=496.4858M 0:7=537.8452M
+ 0:8=555.6659M 0:10=5.0000 0:11=234.3306M
**** VOLTAGE SOURCES
SUBCKT
ELEMENT 0:VNCE 0:VN7 0:VPCE 0:VP7
VOLTS 0 5.00000 0 -5.00000
AMPS -2.07407U -405.41294P 2.07407U 405.41294P
POWER 0. 2.02706N 0.
2.02706N
TOTAL VOLTAGE SOURCE POWER DISSIPATION=4.0541 N WATTS
**** BIPOLAR JUNCTION TRANSISTORS
SUBCKT
ELEMENT
0:QN1 0:QN2
0:QN3 0:QN4
* Note: HSPICE RF does not support qn(element)
* charge output.
MODEL
0:N1
0:N1
0:N1
0:N1
IB 999.99912N 2.00000U 5.00000U 10.00000U
IC -987.65345N -1.97530U -4.93827U -9.87654U
VBE 437.32588M 455.13437M 478.67632M 496.48580M
VCE 437.32588M 17.80849M 23.54195M 17.80948M
VBC 437.32588M 455.13437M 478.67632M 496.48580M
VS 0. 0. 0. 0.
POWER 5.39908N 875.09107N 2.27712U 4.78896U
BETAD -987.65432M -987.65432M -987.65432M -987.65432M
GM 0. 0. 0. 0.
RPI 2.0810E+06 1.0405E+06 416.20796K 208.10396K
RX 250.00000M
250.00000M 250.00000M 250.00000M
RO 2.0810E+06 1.0405E+06 416.20796K 208.10396K
CPI 1.43092N 1.44033N 1.45279N 1.46225N
CMU 954.16927P 960.66843P 969.64689P 977.06866P
CCS 800.00000P 800.00000P 800.00000P 800.00000P
BETAAC 0. 0. 0. 0.
FT
0. 0. 0. 0.
Element Statement IC Parameter
Use the element statement parameter, IC=<val>, to set DC terminal voltages
for selected active devices.
HSPICE uses the value, set in IC=<val>, as the DC operating point value, in
the DC solution.
■
292
HSPICE RF does not support this option, so IC is always set to IC=OFF.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
DC Initialization and Operating Point Calculation
Example
This example describes an H element dependent-voltage source:
HXCC 13 20 VIN1 VIN2 IC=0.5, 1.3
The current, through VIN1, initializes to 0.5 mA. The current, through VIN2,
initializes to 1.3 mA.
Initial Conditions
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.
.NODESET 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.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
293
Chapter 8: Initializing DC/Operating Point Analysis
DC Initialization and Operating Point Calculation
SAVE and LOAD Statements
HSPICE saves the operating point, unless you use the .SAVE LEVEL=NONE
statement. HSPICE restores the saved operating-point file, only if the input file
contains a .LOAD statement.
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.
A parameter or temperature sweep saves only the first operating point.
Note:
HSPICE RF does not support .SAVE and .LOAD statements.
If any node initialization commands, such as .NODESET and .IC, appear in the
netlist after the .LOAD command, then they overwrite the .LOAD initialization. If
you use this feature to set particular states for multistate circuits (such as flipflops), you can still use the .SAVE command to speed up the DC convergence.
.SAVE and .LOAD work even on changed circuit topologies. Adding or deleting
nodes results in a new circuit topology. HSPICE initializes the new nodes, as if
you did not save an operating point. HSPICE ignores references to deleted
nodes, but initializes coincidental nodes to the values that you saved from the
previous run.
When you initialize nodes to voltages, HSPICE inserts Norton-equivalent
circuits at each initialized node. The conductance value of a Norton-equivalent
circuit is GMAX=100, which might be too large for some circuits.
If using .SAVE and .LOAD does not speed up simulation, or causes simulation
problems, use .OPTION GMAX=1e-12 to minimize the effect of Nortonequivalent circuits on matrix conductances.
HSPICE still uses the initialized node voltages to initialize devices. HSPICE RF
does not output node voltage from operating point (.OP), if time (t) < 0.
.SAVE Statement
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
294
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
.DC Statement—DC Sweeps
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.
.LOAD Statement
Use the .LOAD statement to input the contents of a file, that you stored using
the .SAVE statement in HSPICE.
Note:
HSPICE RF does not support the .SAVE and .LOAD (save and restart)
statements.
Files stored with the .SAVE statement contain operating point data for the point
in the analysis at which you executed .SAVE. Do not use the .LOAD command
for concatenated netlist files.
.DC Statement—DC Sweeps
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, using start and stop (HSPICE only; not
supported in HSPICE RF).
■
Perform a DC model characterization (HSPICE only; not supported in
HSPICE RF).
The .DC statement format depends on the application that uses it.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
295
Chapter 8: Initializing DC/Operating Point Analysis
Other DC Analysis Statements
Other DC Analysis Statements
HSPICE or HSPICE RF also provides the following DC analysis statements.
Each statement uses the DC-equivalent model of the circuit in its analysis.
For .PZ, the equivalent circuit includes capacitors and inductors.
Statement
Description
.DCMATCH
(HSPICE) A technique for computing the effects of local variations in
device characteristics on the DC solution of a circuit.
.PZ
Performs pole/zero analysis.
.SENS
(HSPICE) Obtains DC small-signal sensitivities of output variables for
circuit parameters.
.TF
Calculates DC small-signal values for transfer functions (ratio of
output variable, to input source).
HSPICE or HSPICE RF includes DC control options, and DC initialization
statements, to model resistive parasitics and initialize nodes. These statements
enhance convergence properties and accuracy of simulation. This section
describes how to perform DC-related, small-signal analysis.
DC Initialization Control Options
Use control options in a DC operating-point analysis, to control DC
convergence properties and simulation algorithms. Many of these options also
affect transient analysis, because DC convergence is an integral part of
transient convergence. Include the following options for both DC and transient
convergence:
■
Absolute and relative voltages.
■
Current tolerances.
■
Matrix options.
Use .OPTION statements to specify the following options, which control DC
analysis:
296
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
ABSTOL
DV
ITL2
PIVREL
CAPTAB
GDCPATH
KCLTEST
PIVTOL
CSHDC
GRAMP
MAXAMP
RESMIN
DCCAP
GSHDC
NEWTOL
SPARSE
DCFOR
GSHUNT
NOPIV
SYMB
DCHOLD
ICSWEEP
OFF
DCIC
ITLPTRAN
PIVOT
DCSTEP
ITL1
PIVREF
DC and AC analysis also use some of these options. Many of these options
also affect the transient analysis, because DC convergence is an integral part
of transient convergence. For a description of transient analysis, see Chapter 9,
Transient Analysis.
Accuracy and Convergence
Convergence is the ability to solve a set of circuit equations, within specified
tolerances, and within a specified number of iterations. In numerical circuit
simulation, a designer specifies a relative and absolute accuracy for the circuit
solution. The simulator iteration algorithm then attempts to converge to a
solution that is within these set tolerances. That is, if consecutive simulations
achieve results within the specified accuracy tolerances, circuit simulation has
converged. How quickly the simulator converges, is often a primary concern to
a designer—especially for preliminary design trials. So designers willingly
sacrifice some accuracy for simulations that converge quickly.
Accuracy Tolerances
HSPICE or HSPICE RF uses accuracy tolerances that you specify, to assure
convergence. These tolerances determine when, and whether, to exit the
convergence loop. For each iteration of the convergence loop, HSPICE or
HSPICE® Simulation and Analysis User Guide
Y-2006.03
297
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
HSPICE RF subtracts previously-calculated values from the new solution, and
compares the result with the accuracy tolerances.
If the difference between two consecutive iterations is within the specified
accuracy tolerances, the circuit simulation has converged.
| Vnk - Vnk-1 | <=accuracy tolerance
■
Vnk is the solution at the n timepoint for iteration k.
■
Vnk-1 is the solution at the n timepoint for iteration k - 1.
As Table 41 shows, HSPICE or HSPICE RF defaults to specific absolute and
relative values. You can change these tolerances, so that simulation time is not
excessive, but accuracy is not compromised. Accuracy Control Options on
page 299 describes the options in Table 41.
Table 41
Absolute and Relative Accuracy Tolerances
Type
.OPTION
Default
Nodal Voltage Tolerances
ABSVDC
50 μv
RELVDC
.001
ABSI
1 nA
RELI
.01
ABSMOS
1 uA
RELMOS
.05
Current Element Tolerances
HSPICE or HSPICE RF compares nodal voltages and element currents, to the
values from the previous iteration.
■
If the absolute value of the difference is less than ABSVDC or ABSI, then the
node or element has converged.
ABSV and ABSI set the floor value, below which HSPICE or HSPICE RF
ignores values. Values above the floor use RELVDC and RELI as relative
tolerances. If the iteration-to-iteration absolute difference is less than these
tolerances, then it is convergent.
Note:
ABSMOS and RELMOS are the tolerances for MOSFET drain currents.
298
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
Accuracy settings directly affect the number of iterations before convergence.
■
If accuracy tolerances are tight, the circuit requires more time to converge.
■
If the accuracy setting is too loose, the resulting solution can be inaccurate
and unstable.
Table 42 shows an example of the relationship between the RELVDC value, and
the number of iterations.
Table 42
RELV vs. Accuracy and Simulation Time for 2 Bit Adder
RELVDC
Iteration
Delay (ns)
Period (ns)
Fall time (ns)
.001
540
31.746
14.336
1.2797
.005
434
31.202
14.366
1.2743
.01
426
31.202
14.366
1.2724
.02
413
31.202
14.365
1.3433
.05
386
31.203
14.365
1.3315
.1
365
31.203
14.363
1.3805
.2
354
31.203
14.363
1.3908
.3
354
31.203
14.363
1.3909
.4
341
31.202
14.363
1.3916
.4
344
31.202
14.362
1.3904
Accuracy Control Options
The default control option settings are designed to maximize accuracy, without
significantly degrading performance. For a description of these options and
their settings, see Simulation Speed and Accuracy on page 327.
ABSH
DCON
RELH
ABSI
DCTRAN
RELI
ABSMOS
DI
RELMOS
HSPICE® Simulation and Analysis User Guide
Y-2006.03
299
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
ABSVDC
GMAX
RELV
CONVERGE
GMINDC
RELVDC
Autoconverge Process
If a circuit does not converge in the number of iterations that ITL1 specifies,
HSPICE or HSPICE RF initiates an auto-convergence process. This process
manipulates DCON, GRAMP, and GMINDC, and even CONVERGE in some cases.
Figure 37 on page 301 shows the autoconverge process.
Note:
HSPICE uses autoconvergence in transient analysis, but it also uses
autoconvergence in DC analysis if the Newton-Raphson (N-R) method fails
to converge.
300
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
Figure 37
Autoconvergence Process Flow Diagram
Start
STEP 1
Iterates up to the ITL1 limit.
Iterate
Y
Results
Converged?
N
STEP 2
Sets DCON=1.
If DV = 1000, sets DV from 1000 to max(0.1. Vmax/50).
Sets GRAMP=(Imax/GMINDC).
Ramps GMINDC, from GMINDC⋅10GRAMP to 1e-12.
Try DCON=1
Converged?
Y
STEP 3
Sets DCON=2.
Relaxes DV to 1e6.
Sets GRAMP=(Imax/GMINDC).
Ramps GMINDC, from GMINDC⋅10GRAMP to 1e-12.
N
Try DCON=2
Converged?
Y
N
Try CONVERGE=1
Converged?
Results
Y
N
Try CONVERGE=4
Results
STEP 4
Adds CSHDC and GSHUNT, from each node, to ground.
Ramps supplies, from zero to the set values.
Removes CSHDC and GSHUNT, after DC convergence.
Also iterates to a stable DC-bias point.
Results
STEP 5
Adds CSHDC, from each node, to ground.
Ramps gmath=cshdc/delta in the range of 1.0e-12 to 10.0.
Set gmath to zero, if convergence occurs with gmath under
1.0e-12, and iterates further to a stable DC bias point.
Y
Converged?
Results
N
Non-convergence report
In Figure 37 above:
■
Setting .OPTION DCON=-1 disables steps 2 and 3.
■
Setting .OPTION CONVERGE=-1 disables steps 4 and 5.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
301
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
■
Setting .OPTION DCON=-1 CONVERGE=-1 disables steps 2, 3, 4, and 5.
■
If you set the DV option to a value other than the default, step 2 uses the
value you set for DV, but step 3 changes DV to 1e6.
■
Setting .OPTION GRAMP has no effect on autoconverge. Autoconverge sets
GRAMP independently.
■
If you set .OPTION GMINDC, then GMINDC ramps to the value you set,
instead of to 1e-12, in steps 2 and 3.
DCON and GMINDC
The GMINDC option helps stabilize the circuit, during DC operating-point
analysis. For MOSFETs, GMINDC helps stabilize the device in the vicinity of the
threshold region. HSPICE or HSPICE RF inserts GMINDC between:
■
Drain and bulk.
■
Source and bulk.
■
Drain and source.
The drain-to-source GMINDC helps to:
■
Linearize the transition from cutoff to weakly-on.
■
Smooth-out model discontinuities.
■
Compensate for the effects of negative conductances.
The pn junction insertion of GMINDC in junction diodes linearizes the low
conductance region. As a result, the device behaves like a resistor in the lowconductance region. This prevents the occurrence of zero conductance, and
improves the convergence of the circuit.
If a circuit does not converge, HSPICE or HSPICE RF automatically sets the
DCON option. This option invokes GMINDC ramping, in steps 2 and 3 of
Figure 37.
GMINDC for various elements is shown in Figure 38 on page 303.
302
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Accuracy and Convergence
Figure 38
GMINDC Insertion
GMINDC
Diode element
GMINDC
BJT element
GMINDC
GMINDC
MOSFET element
GMINDC
GMINDC
JFET or MESFET
element
GMINDC
HSPICE® Simulation and Analysis User Guide
Y-2006.03
303
Chapter 8: Initializing DC/Operating Point Analysis
Reducing DC Errors
Reducing DC Errors
To reduce DC errors, perform the following steps:
1. To check topology, set .OPTION NODE, to list nodal cross-references.
•
Do all MOS p-channel substrates connect to either VCC or positive
supplies?
•
Do all MOS n-channel substrates connect to either GND or negative
supplies?
•
Do all vertical NPN substrates connect to either GND or negative
supplies?
•
Do all lateral PNP substrates connect to negative supplies?
•
Do all latches have either an OFF transistor, a .NODESET, or an .IC,
on one side?
•
Do all series capacitors have a parallel resistance, or is .OPTION
DCSTEP set?
2. Check your .MODEL statements.
304
•
Check all model parameter units. Use model printouts to verify actual
values and units, because HSPICE multiplies some model parameters
by scaling options.
•
Are sub-threshold parameters of MOS models, set with reasonable
value (such as NFS=1e11 for SPICE 1, 2, and 3 models, or N0=1.0 for
HSPICE BSIM1, BSIM2, and Level 28 device models)?
•
Do not set UTRA in MOS Level 2 models.
•
Are JS and JSW set in the MOS model for the DC portion of a diode
model? A typical JS value is 1e-4A/M2.
•
Are CJ and CJSW set, in MOS diode models?
•
Is weak-inversion NG and ND set in JFET/MESFET models?
•
If you use the MOS Level 6 LGAMMA equation, is UPDATE=1?
•
Make sure that DIODE models have non-zero values for saturation
current, junction capacitance, and series resistance.
•
Use MOS ACM=1, ACM=2, or ACM=3 source and drain diode
calculations, to automatically generate parasitics.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Reducing DC Errors
3. General remarks:
•
Ideal current sources require large values of .OPTION GRAMP,
especially for BJT and MESFET circuits. Such circuits do not ramp up
with the supply voltages, and can force reverse-bias conditions, leading
to excessive nodal voltages.
•
Schmitt triggers are unpredictable for DC sweep analysis, and
sometimes for operating points for the same reasons that oscillators and
flip-flops are unpredictable. Use slow transient.
•
Large circuits tend to have more convergence problems, because they
have a higher probability of uncovering a modeling problem.
•
Circuits that converge individually, but fail when combined, are almost
guaranteed to have a modeling problem.
•
Open-loop op-amps have high gain, which can lead to difficulties in
converging. Start op-amps in unity-gain configuration, and open them
up in transient analysis, using a voltage-variable resistor, or a resistor
with a large AC value (for AC analysis).
4. Check your options:
•
Remove all convergence-related options, and try first with no
special .OPTION settings.
•
Check non-convergence diagnostic tables for non-convergent nodes.
Look up non-convergent nodes in the circuit schematic. They are
usually latches, Schmitt triggers, or oscillating nodes.
•
For stubborn convergence failures, bypass DC all together, and
use .TRAN with UIC set. Continue transient analysis until transients
settle out, then specify the .OP time, to obtain an operating point during
the transient analysis. To specify an AC analysis during the transient
analysis, add an .AC statement to the .OP time statement.
•
SCALE and SCALM scaling options have a significant effect on
parameter values in both elements and models. Be careful with units.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
305
Chapter 8: Initializing DC/Operating Point Analysis
Reducing DC Errors
Shorted Element Nodes
HSPICE or HSPICE RF disregards any capacitor, resistor, inductor, diode, BJT,
or MOSFET, if all of its leads connect together. Simulation does not count the
component in its component tally, and issues a warning:
** warning **
all nodes of element x:<name> are connected together
Inserting Conductance, Using DCSTEP
In a DC operating-point analysis, failure to include conductances in a capacitor
model results in broken circuit loops (because a DC analysis opens all
capacitors). This might not be solvable. If you include a small conductance in
the capacitor model, the circuit loops are complete, and HSPICE or HSPICE
RF can solve them.
Modeling capacitors as complete opens, can result in this error:
“No DC Path to Ground”
For a DC analysis, use .OPTION DCSTEP, to assign a conductance value to
all capacitors in the circuit. DCSTEP calculates the value as:
conductance=capacitance/DCSTEP
In Figure 39 on page 307, HSPICE or HSPICE RF inserts conductance (G), in
parallel with capacitance (Cg). This provides current paths around
capacitances, in DC analysis.
306
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
Figure 39
Conductance Insertion
Cg
original circuit
Cg
G
after conductance
insertion
G
G
G
G = Cg/DCSTEP
Floating-Point Overflow
If MOS conductance is negative or zero, HSPICE or HSPICE RF might have
difficulty converging. An indication of this type of problem is a floating-point
overflow, during matrix solutions. HSPICE or HSPICE RF detects floating-point
overflow, and invokes the Damped Pseudo Transient algorithm (CONVERGE=1),
to try to achieve DC convergence without requiring you to intervene. If GMINDC
is 1.0e-12 or less when a floating-point overflows, HSPICE or HSPICE RF sets
it to 1.0e-11.
Diagnosing Convergence Problems
Before simulation, HSPICE or HSPICE RF diagnoses potential convergence
problems in the input circuit, and provides an early warning, to help you in
debugging your circuit. If HSPICE or HSPICE RF detects a circuit condition that
might cause convergence problems, it prints the following message into the
output file:
“Warning: Zero diagonal value detected at node ( ) in
equation solver, which might cause convergence problems.
If your simulation fails, try adding a large resistor
between node ( ) and ground.”
HSPICE® Simulation and Analysis User Guide
Y-2006.03
307
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
Non-Convergence Diagnostic Table
If a circuit cannot converge, HSPICE or HSPICE RF automatically generates
two printouts, called the diagnostic tables:
■
Nodal voltage printout: Prints the names of all no-convergent node voltages,
and the associated voltage error tolerances (tol).
■
Element printout: Lists all non-convergent elements, and their associated
element currents, element voltages, model parameters, and current error
tolerances (tol).
To locate the branch current or nodal voltage that causes non-convergence,
use the following steps:
1. Analyze the diagnostic tables. Look for unusually large values of branch
currents, nodal voltages or tolerances.
2. After you locate the cause, use the .NODESET or .IC statements, to
initialize the node or branch.
If circuit simulation does not converge, HSPICE or HSPICE RF
automatically generates a non-convergence diagnostic table, indicating:
•
The quantity of recorded voltage failures.
•
The quantity of recorded branch element failures.
Any node in a circuit can create voltage failures, including hidden nodes
(such as extra nodes that parasitic resistors create).
3. Check the element printout for the subcircuit, model, and element name for
all parts of the circuit where node voltages or currents do not converge.
For example, Table 43 on page 309 identifies the xinv21, xinv22, xinv23, and
xinv24 inverters, as problem sub-circuits in a ring oscillator. It also indicates
that the p-channel transistors, in the xinv21, xinv22, xinv24 sub-circuits, are
nonconvergent elements. The n-channel transistor of xinv23 is also a
nonconvergent element.
The table lists voltages and currents for the transistors, so you can check
whether they have reasonable values. The tolds, tolbd, and tolbs error
tolerances indicate how close the element currents (drain to source, bulk to
drain, and bulk to source) are, to a convergent solution. For tol variables, a
value close to or below 1.0 is a convergent solution. In Table 43, the tol values
that are around 100, indicate that the currents were far from convergence. The
element current and voltage values are also shown (id, ibs, ibd, vgs, vds, and
308
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
vbs). Examine whether these values are realistic, and determine the transistor
regions of operation.
Table 43
Subcircuit Voltage, Current, and Tolerance
subckt
element
model
xinv21
21:mphc1
0:p1
xinv22
22:mphc1
0:p1
xinv23
23:mphc1
0:p1
xinv23
23:mnch1
0:n1
xinv24
24: mphc1
0:p1
id
27.5809f
140.5646u
1.8123p
1.7017m
5.5132u
ibs
205.9804f
3.1881f
31.2989f
0.
200.0000f
ibd
0.
0.
0.
-168.7011f
0.
vgs
4.9994
-4.9992
69.9223
4.9998
-67.8955
vds
4.9994
206.6633u
69.9225
-64.9225
2.0269
vbs
4.9994
206.6633u
69.9225
0.
2.0269
vth
-653.8030m
-745.5860m
-732.8632m
549.4114m
-656.5097m
tolds
114.8609
82.5624
155.9508
104.5004
5.3653
tolbd
0.
0.
0.
0.
0.
tolbs
3.534e-19
107.1528m
0.
0.
0.
Traceback of Non-Convergence Source
To locate a non-convergence source, trace the circuit path for error tolerance.
For example, in an inverter chain, the last inverter can have a very high error
tolerance. If this is the case, examine the error tolerance of the elements that
drive the inverter. If the driving tolerance is high, the driving element could be
the source of non-convergence. However, if the tolerance is low, check the
driven element as the source of non-convergence.
Examine the voltages and current levels of a non-convergent MOSFET to
discover the operating region of the MOSFET. This information can flow to the
location of the discontinuity in the model—for example, subthreshold-to-linear,
or linear-to-saturation.
When considering error tolerances, check the current and nodal voltage values.
If these values are extremely low, a relatively large number is divided by a very
HSPICE® Simulation and Analysis User Guide
Y-2006.03
309
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
small number. This produces a large calculation result, which can cause the
non-convergence errors. To solve this, increase the value of the absoluteaccuracy options.
Use the diagnostic table, with the DC iteration limit (ITL1 option), to find the
sources of non-convergence. When you increase or decrease ITL1, HSPICE
or HSPICE RF prints output for the problem nodes and elements for a new
iteration—that is, the last iteration of the analysis that you set in ITL1.
Solutions for Non-Convergent Circuits
Non-convergent circuits generally result from:
■
Poor Initial Conditions
■
Inappropriate Model Parameters
■
PN Junctions (Diodes, MOSFETs, BJTs)
The following sections explain these conditions.
Poor Initial Conditions
Multi-stable circuits need state information, to guide the DC solution. You must
initialize ring oscillators and flip-flops. These multi-stable circuits can either
produce an intermediate forbidden state, or cause a DC convergence problem.
To initialize a circuit, use the .IC statement, which forces a node to the
requested voltage. Ring oscillators usually require you to set only one stage.
Figure 40
Ring Oscillator
.IC V(1)=5V
1
2
3
4
5
The best way to set up the flip-flop is to use an .IC statement in the subcircuit
definition.
310
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
Example
The following example sets the local Qset parameter to 0, and uses this value
for the .IC statement, to initialize the Q latch output node. As a result, all
latches have a default state of Q low. Setting Qset to vdd calls a latch, which
overrides this state.
.subckt latch in Q Q/ d Qset=0
.ic Q=Qset
...
.ends
Xff data_in[1] out[1] out[1]/ strobe LATCH Qset=vdd
Inappropriate Model Parameters
If you impose non-physical model parameters, you might create a
discontinuous IDS or capacitance model. This can cause an internal timestep
too small error, during the transient simulation. The mosivcv.sp demonstration
file shows IDS, VGS, GM, GDS, GMB, and CV plots for MOS devices. A sweep
near threshold, from Vth-0.5 V to Vth+0.5 V (using a delta of 0.01 V),
sometimes discloses a possible discontinuity in the curves.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
311
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
Figure 41
Discontinuous I-V Characteristics
Ids
I-V characteristics exhibiting
saturation conductance = zero
Vds
Ids
I-V exhibiting VDSAT slope error
Vds
Ids
I-V exhibiting negative resistance region
Vds
If simulation does not converge when you add a component or change a
component value, then the model parameters are not appropriate or do not
correspond to physical values they represent.
To locate the problem, follow these steps:
1. Check the input netlist file for non-convergent elements.
Devices with a TOL value greater than 1, are non-convergent.
2. Find the devices at the beginning of the combined-logic string of gates that
seem to start the non-convergent string.
312
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
3. Check the operating point of these devices very closely, to see what region
they operate in.
Model parameters associated with this region are probably inappropriate.
Circuit simulation uses single-transistor characterization, to simulate a large
collection of devices. If a circuit fails to converge, the cause can be a single
transistor, anywhere in the circuit.
PN Junctions (Diodes, MOSFETs, BJTs)
PN junctions found in diode, BJT, and MOSFET models, might exhibit nonconvergent behavior, in both DC and transient analysis.
Example
PN junctions often have a high off resistance, resulting in an ill-conditioned
matrix. To overcome this, use .OPTION GMINDC and .OPTION GMIN to
automatically parallel every PN junction in a design, with a conductance.
Non-convergence can occur if you overdrive the PN junction. This happens if
you omit a current-limiting resistor, or if the resistor has a very small value. In
transient analysis, protection diodes are often temporarily forward-biased (due
to the inductive switching effect). This overdrives the diode, and can result in
non-convergence, if you omit a current-limiting resistor.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
313
Chapter 8: Initializing DC/Operating Point Analysis
Diagnosing Convergence Problems
314
HSPICE® Simulation and Analysis User Guide
Y-2006.03
9
9
Transient Analysis
Describes how to use transient analysis to compute the circuit solution.
Transient analysis computes the circuit solution, as a function of time, over a
time range specified in the .TRAN statement.
For descriptions of individual HSPICE commands referenced in this chapter,
see the HSPICE Command Reference.
Simulation Flow
Figure 42 illustrates the simulation flow for transient analysis in Synopsys
HSPICE and HSPICE RF.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
315
Chapter 9: Transient Analysis
Overview of Transient Analysis
Figure 42
Transient Analysis Simulation Flow
Simulation Experiment
Transient
DC
UIC
.FOUR
.OPTION:
Method
BYPASS
CSHUNT
DVDT
GSHUNT
LVLTIM=x
MAXORD=x
METHOD
RUNLVL=x
AC
Time-sweep
simulation
.FFT
HSPICE only
Tolerance
ABSV=x
ABSVAR=x
ACCURATE
BYTOL=x
CHGTOL=x
DELMAX=x
FAST
MBYPASS
MU
Limit
RELQ=x
RELTOL
RELV=x
RELVAR=x
SLOPETOL=x
TIMERES
TRTOL=x
VNTOL
AUTOSTOP
BKPSIZ
DVTR=x
FS=x
FT=x
GMIN=x
IMAX=x
IMIN=x
ITL3=x
ITL4=x
ITL5=x
RMAX=x
RMIN=x
VFLOOR
Overview of Transient Analysis
Transient analysis simulates a circuit at a specific time. Some of its algorithms,
control options, convergence-related issues, and initialization parameters are
different than those used in DC analysis. However, a transient analysis first
performs a DC operating point analysis, unless you specify the UIC option in
the .TRAN statement. Therefore, most DC analysis algorithms, control options,
initialization issues, and convergence issues, also apply to transient analysis.
Unless you set the initial circuit operating conditions, some circuits (such as
oscillators, or circuits with feedback) do not have stable operating point
solutions. For these circuits, either:
316
■
Break the feedback loop, to calculate a stable DC operating point, or
■
Specify the initial conditions, in the simulation input.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Overview of Transient Analysis
If you include the UIC parameter in the .TRAN statement, HSPICE or HSPICE
RF bypasses the DC operating point analysis. Instead, it uses node voltages,
specified in an .IC statement, to start a transient analysis. For example, if
a .IC statement sets a node to 5 V in, the value at that node for the first time
point (time 0) is 5 V.
You can use the .OP statement to store an estimate of the DC operating point,
during a transient analysis.
Example
In the following example, the UIC parameter (in the .TRAN statement)
bypasses the initial DC operating point analysis. The .OP statement calculates
the transient operating point (at t=20 ns), during the transient analysis.
.TRAN 1ns 100ns UIC
.OP 20ns
Although a transient analysis might provide a convergent DC solution, the
transient analysis can still fail to converge. In a transient analysis, the internal
timestep too small error message indicates that the circuit failed to converge.
The cause of this convergence failure might be that stated initial conditions are
not close enough to the actual DC operating point values. Use the commands
in this chapter to help achieve convergence in a transient analysis.
Transient Analysis Output
.print tran ov1 [ov2 ... ovN]
.probe tran ov1 [ov2 ... ovN]
.measure tran measspec
.plot tran ov1 [ov2 ... ovN]
.graph tran ov1 [ov2 ... ovN]
HSPICE RF does not support .PLOT or .GRAPH.
The ov1, ... ovN output variables can include the following:
■
V(n): voltage at node n.
■
V(n1<,n2>): voltage between the n1 and n2 nodes.
■
Vn(d1): voltage at nth terminal of the d1 device.
■
In(d1): current into nth terminal of the d1 device.
■
‘expression’: expression, involving the plot variables above
HSPICE® Simulation and Analysis User Guide
Y-2006.03
317
Chapter 9: Transient Analysis
Overview of Transient Analysis
You can use wildcards (*), or as specified in the .hspicerf configuration file) to
specify multiple output variables in a single command. Output is affected by
.OPTION POST or .OPTION PROBE, SIM_DELTAI, and SIM_DELTAV.
Parameter
*.print
Description
Writes the output from the .PRINT statement to a *.print file. HSPICE
does not generate a *.print# file.
■
■
■
■
*.tr#
The header line contains column labels.
The first column is time.
The remaining columns represent the output variables specified
with .PRINT.
Rows that follow the header contain the data values for simulated
time points.
Writes output from the .PROBE, .PRINT, .PLOT, .GRAPH,
or .MEASURE statement to a *.tr# file.
Transient Analysis of an RC Network
Follow these steps to run a transient analysis of a RC network with a pulse
source, a DC source, and an AC source:
1. Type the following netlist into a file named quickTRAN.sp.
A SIMPLE TRANSIENT RUN
.OPTION LIST NODE POST
.OP
.TRAN 10N 2U
.PRINT TRAN V(1) V(2) I(R2) I(C1)
V1 1 0 10 AC 1 PULSE 0 5 10N 20N 20N 500N 2U
R1 1 2 1K
R2 2 0 1K
C1 2 0 .001U
.END
This example is based on demonstration netlist quickTRAN.sp, which is
available in directory $<installdir>/demo/hspice/apps:
A SIMPLE TRANSIENT RUN
.OPTION LIST NODE POST
.OP
.TRAN 10N 2U
.PRINT TRAN V(1) V(2) I(R2) I(C1)
V1 1 0 10 AC 1 PULSE 0 5 10N 20N 20N 500N 2U
318
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Overview of Transient Analysis
R1 1 2 1K
R2 2 0 1K
C1 2 0 .001U
.END
Note:
The V1 source specification includes a pulse source. For the syntax of
pulse sources and other types of sources, see Chapter 5, Sources and
Stimuli.
2. To run HSPICE, type the following:
hspice quickTRAN.sp > quickTRAN.lis
3. To examine the simulation results and status, use an editor and view the .lis
and .st0 files.
4. Run AvanWaves and open the .sp file.
5. To view the waveform, select the quickTRAN.tr0 file from the Results
Browser window.
6. Display the voltage at nodes 1 and 2 on the x-axis.
Figure 43 shows the waveforms.
Figure 43
Voltages at RC Network Circuit Node 1 and Node 2
A simple transient
5.0
4.0
3.0
2.0
1.0
0.
0.
200.0n
400.0n
600.0n
800.0n 1.0u
1.20u
time CL(n)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
1.40u
1.60u
1.80u
2.0u
319
Chapter 9: Transient Analysis
Overview of Transient Analysis
Transient Analysis of an Inverter
As a final example, you can analyze the behavior of the simple MOS inverter
shown in Figure 44.
Figure 44
MOS Inverter Circuit
VCC
VCC
+
_
M1
IN
VIN
OUT
CLOAD
0.75 pF
+
_
M2
Follow these steps to analyze this behavior:
1. Type the following netlist data into a file named quickINV.sp.
Inverter Circuit
.OPTION LIST NODE POST
.TRAN 200P 20N
.PRINT TRAN V(IN) V(OUT)
M1 OUT IN VCC VCC PCH L=1U W=20U
M2 OUT IN 0 0 NCH L=1U W=20U
VCC VCC 0 5
VIN IN 0 0 PULSE .2 4.8 2N 1N 1N 5N 20N
CLOAD OUT 0 .75P
.MODEL PCH PMOS LEVEL=1
.MODEL NCH NMOS LEVEL=1
.END
You can find the complete netlist for this example in directory $<installdir>/
demo/hspice/apps/quickINV.sp.
2. To run HSPICE, type the following:
hspice quickINV.sp > quickINV.lis
3. Use AvanWaves to examine the voltage waveforms, at the inverter IN and
OUT nodes.
320
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Using the .BIASCHK Statement
Figure 45 shows the waveforms.
Figure 45
Voltage at MOS Inverter Node 1 and Node 2
Inverter Circuit
04/21/2003 16.48.25
1
5.0
Volt (lin)
4.0
Input
quickinv.t
in
out
Output
3.0
2.0
1.0
0
0
2.0
4.0
6.0
8.0
10.0
time (lin)
12.0
14.0
16.0
18.0
20.0
Using the .BIASCHK Statement
The .BIASCHK statement can monitor the voltage bias, current, device-size,
expression and region during transient analysis, and reports:
■
Element name
■
Time
■
Terminals
■
Bias that exceeds the limit
■
Number of times the bias exceeds the limit for an element
For the syntax and description of this statement, see the .BIASCHK command
in the HSPICE Command Reference.
HSPICE or HSPICE RF saves the information as both a warning and a
BIASCHK summary in the *.lis file. You can use this command only for active
elements and capacitors.
You can also use .OPTION BIASFILE and .OPTION BIAWARN with
a .BIASCHK statement.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
321
Chapter 9: Transient Analysis
Using the .BIASCHK Statement
The following limitations apply to the .BIASCHK statement:
■
.BIASCHK is only supported for diode, jfet, nmos, pmos, bjt, and c models,
as well as subcircuits.
■
For a device-size check, only W and L MOSFET models are supported.
■
Wildcards in element and model names, and except definitions are
supported but not in expressions.
Data Checking Methods
Four methods are available to check the data with the .BIASCHK command:
■
Limit and noise method
■
Maximum method
■
Minimum method
■
Region method
Note:
The region method of data checking is only supported in MOSFET
models.
Limit and Noise Method
For a transient simulation using the limit and noise method to check the data,
use the following syntax:
For local_max
v(tn-1) > limit_value
The bias corresponds anyone of the following two conditions:
■
v(tn-1) > v(tn) && v(tn-1) >= v(tn-2)
■
v(tn-1) >= v(tn) && v(tn-1) > v(tn-2)
local_min: The minimum bias after the time last local max occurs.
During a transient analysis, the local_max is recorded if it is greater than the
limit. In the summary reported after transient analysis, the
local_max(current) is replaced with the local_max(next) when the
following comparison is true:
local_max(current) - local_min < noise && local_max(next) - local_min < noise
&& local_max(current) < local_max(next)
322
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Using the .BIASCHK Statement
At the end of the simulation, all local_max values are listed as BIASCHK
warnings. During other analyses, warnings are issued when the value you want
to check is greater than the limit_value you specify.
Maximum Method
For a transient simulation using the maximum method to check the data, use
the following syntax:
For local_max:
v(tn-1) > max_value
The bias corresponds any one of the following two conditions:
■
v(tn-1) > v(tn) && v(tn-1) >= v(tn-2)
■
v(tn-1) >= v(tn) && v(tn-1) > v(tn-2)
During a transient analysis, all local_max values are listed as BIASCHK
warnings. During other analyses, warnings are issued when the value you want
to check is greater than max_value you specify.
Minimum Method
For a transient simulation using the minimum method to check the data, use the
following syntax:
For local_min:
v(tn) < min_value
The bias corresponds any one of the following two conditions:
■
v(tn-1) < v(tn) && v(tn-1) <= v(tn-2)
■
v(tn-1) <= v(tn) && v(tn-1) < v(tn-2)
During a transient analysis, all local_min values are listed as BIASCHK
warnings. During other analyses, warnings are issued when the value you want
to check is smaller than min_value you specify.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
323
Chapter 9: Transient Analysis
Using the .BIASCHK Statement
Region Method
This method is only for MOSFET models. Three regions exist:
■
cutoff
■
linear
■
saturation
When the specified transistor enters and exits during transient analysis, the
specified region is reported.
Example
The following example is a netlist that uses the .BIASCHK command for a
transient simulation. This example is based on demonstration netlist
biaschk.sp, which is available in directory $<installdir>/demo/hspice/apps:
* Test Case
* Transient simulation
.Tran 1n 8n
.Options Post NoMod biasfile = 'result'
.biaschk nmos terminal1=nd terminal2=nb max=.006
.biaschk nmos terminal1=nb terminal2=ns limit=.006
+ noise=.005
.biaschk mos region=saturation region=linear mname=nmos
+ mname=pmos
.biaschk c terminal1=n1 max=.1
+ name='c10','c14','c15','c8','c7'
.biaschk 'v(net27)-v(net25)' min=.1e-10 max=1 simu=all
+ $monitor=op monitor=dc monitor=tr
.biaschk 'v(net25)-v(0)' min=.1e-5 max='0.1*v(net31)'
+ simu=tran
.biaschk mos terminal1=nb monitor = l mname=nmos
+ simulation = tran min=1u
.biaschk mos terminal1=nb monitor = w mname=nmos
+ simulation = tran min =10u
.biaschk mos terminal1=nb monitor = i mname=nmos simu = op
+ simu=tran max = 1m
.biaschk 'v(net25)' min=2.5 tstart=2n tstop=6n $autostop
v28 data gnd PWL 0s 5v 1n 5v 2n 0v
v27 clock gnd PWL 0s 0v 3n 0v 4n 5v
.model nmos nmos level=2
.model pmos pmos level=2
.Global vdd gnd
.subckt XGATE control in n_control out
m0 in n_control out vdd pmos l=1.2u w=3.4u
m1 in control out gnd nmos l=1.2u w=3.4u
.ends
.subckt INV in out wp=9.6u wn=4u l=1.2u
324
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Transient Control Options
mb2 out in gnd gnd nmos l=l w=wn
mb1 out in vdd vdd pmos l=l w=wp
.ends
.subckt DFF c d nc nq
Xi64 nc net46 c net36 XGATE
Xi66 nc net38 c net39 XGATE
Xi65 c nq nc net36 XGATE
Xi62 c d nc net39 XGATE
Xi60 net722 nq INV
Xi61 net46 net38 INV
Xi59 net36 net722 INV
Xi58 net39 net46 INV
c20 net36 gnd c=17f
c15 net39 gnd c=15f
c12 net46 gnd c=25f
c4 nq gnd c=25f
c3 net722 gnd c=19f
c16 net38 gnd c=16f
.ends
*---------------------------------------------------* Main Circuit Netlist:
*--------------------------------------------------------v14 vdd gnd dc=5
c10 vdd gnd c=35f
c15 d_output gnd c=21f
c12 dff_nq gnd c=11f
c11 net31 gnd c=42f
c14 net27 gnd c=34f
c13 net25 gnd c=41f
c8 clock gnd c=5f
c7 data gnd c=7f
Xi3 net25 net31 net27 dff_nq DFF l=1u wn=3.8u wp=10u
Xi6 data net31 INV
Xi5 net25 net27 INV
Xi4 clock net25 INV
Xi2 dff_nq d_output INV wp=26.4u wn=10.6u
.print v(clock) v(net25)
.op
.end
Transient Control Options
Method, tolerance, and limit options in this section modify the behavior of
transient analysis integration routines. Delta is the internal timestep. TSTEP
and TSTOP are the step and stop values in the .TRAN statement. Asterisk
denotes an option only available in HSPICE RF (not supported in HSPICE).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
325
Chapter 9: Transient Analysis
Transient Control Options
Table 44
Transient Control Options, Arranged by Category
Method
Tolerance
BYPASS
CSHUNT
DVDT
GSHUNT
INTERP
ITRPRT
LVLTIM
MAXORD
METHOD
POST*
PROBE*
PURETP
SIM_ORDER*
RUNLVL
SIM_TRAP*
TRCON
ABSH
ABSV
ABSVAR
ACCURATE
BYTOL
CHGTOL
DI
FAST
MBYPASS
MAXAMP
MU
RELH
RELI
RELQ
RELTOL
RELV
Limit
RELVAR
SIM_ACCURACY*
SIM_DELTAI*
SIM_DELTAV*
SLOPETOL
TIMERES
TRTOL
VNTOL
AUTOSTOP
BKPSIZ
DELMAX
DVTR
FS
FT
GMIN
ITL3
ITL4
ITL5
RMAX
RMIN
VFLOOR
Matrix Manipulation Options
After HSPICE generates individual linear elements in an input netlist, it
constructs linear equations for the matrix. You can set variables that affect how
HSPICE constructs and solves the matrix equation, including .OPTION PIVOT
and .OPTION GMIN (HSPICE RF does not support these options). GMIN
places a variable in the matrix, so the matrix does not become ill-conditioned.
.OPTION PIVOT selects a pivoting method, which reduces simulation time,
and assists in DC and transient convergence. Pivoting reduces errors, resulting
from elements in the matrix that are widely different in magnitude. PIVOT
searches the matrix, to find the largest element value, and uses this value as
the pivot.
326
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Simulation Speed and Accuracy
Simulation Speed and Accuracy
Convergence is the ability to solve a set of circuit equations within specified
tolerances and within a specified number of iterations. In numerical circuit
simulation, you can specify relative and absolute accuracy for the circuit
solution. The simulator iteration algorithm attempts to converge to a solution
that is within these set tolerances. If consecutive simulations achieve results
within the specified accuracy tolerances, circuit simulation has converged. How
quickly the simulator converges, is often a primary concern to a designer—
especially for preliminary design trials. So designers willingly sacrifice some
accuracy for simulations that converge quickly.
Simulation Speed
HSPICE or HSPICE RF can substantially reduce the computer time needed to
solve complex problems. Use the following options to alter the internal
algorithms to increase simulation efficiency.
■
.OPTION FAST – sets additional options, which increase simulation speed,
with minimal loss of accuracy
■
.OPTION AUTOSTOP – terminates the simulation, after completing
all .MEASURE statements. This is of special interest, when testing corners.
Simulation Accuracy
In HSPICE or HSPICE RF, the default control option values aim for superior
accuracy, within an acceptable amount of simulation time. The control options
and their default settings (to maximize accuracy) are:
DVDT=4
LVLTIM=1
RMAX=5
SLOPETOL=0.75
FT=FS=0.25
BYPASS=1
BYTOL=MBYPASS x VNTOL=0.100m
Note:
BYPASS is on (set to 1), only when DVDT=4. For other DVDT settings,
BYPASS is off (0). The SLOPETOL value is 0.75, only if DVDT=4 and
LVLTIM=1. For all other values of DVDT or LVLTIM, SLOPETOL defaults to
0.5.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
327
Chapter 9: Transient Analysis
Simulation Speed and Accuracy
Timestep Control for Accuracy
The DVDT control option selects the timestep control algorithm. For a
description of the relationships between DVDT and other control options, see
Selecting Timestep Control Algorithms on page 333.
The DELMAX control option also affects simulation accuracy. DELMAX specifies
the maximum timestep size. If you do not set .OPTION DELMAX, HSPICE or
HSPICE RF computes a DELMAX value. Factors that determine the computed
DELMAX value are:
■
.OPTION RMAX and .OPTION FS.
■
Breakpoint locations for a PWL source.
■
Breakpoint locations for a PULSE source.
■
Smallest period for a SIN source.
■
Smallest delay for a transmission line component.
■
Smallest ideal delay for a transmission line component.
■
TSTEP value, in a .TRAN analysis.
■
Number of points, in an FFT analysis (HSPICE only).
Use the FS and RMAX control options, to control the DELMAX value.
■
.OPTION FS, which defaults to 0.25, scales the breakpoint interval in the
DELMAX calculation.
■
.OPTION RMAX defaults to 5 (if DVDT=4 and LVLTIM=1), and scales the
TSTEP (timestep) size in the DELMAX calculation.
For circuits that contain oscillators or ideal delay elements, use .OPTION
DELMAX, to set DELMAX to one-hundredth of the period or less.
.OPTION ACCURATE tightens the simulation options to output the most
accurate set of simulation algorithms and tolerances. If you set ACCURATE to 1,
HSPICE or HSPICE RF uses these control options:
Table 45
DVDT=2
BYTOL=0
328
Control Option Settings When ACCURATE=1
RELVAR=0.2LVL BYPASS=0
TIM=3
ABSVAR=0.2
FT=FS=0.2
RMAX=2
RELMOS=0.01
SLOPETOL=0.5
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Simulation Speed and Accuracy
Models and Accuracy
Simulation accuracy depends on the sophistication and accuracy of the models
you use. Advanced MOS, BJT, and GaAs models provide superior results for
critical applications.
The following model types increase simulation accuracy:
■
Algebraic models, which describe parasitic interconnect capacitances as a
function of the width of the transistor. The wire model extension of the
resistor can model the metal, diffusion, or poly interconnects, to preserve
the relationship between the physical layout and the electrical property.
■
The ACM parameter in MOS models, which calculates source and drain
junction parasitic defaults. ACM equations calculate:
•
size of the bottom wall
•
length of the sidewall diodes
•
length of a lightly doped structure.
SPICE defaults do not calculate the junction diode. Specify AD, AS, PD,
PS, NRD, and NRS to override the default calculations.
■
CAPOP=4 models the most advanced charge conservation, non-reciprocal
gate capacitances. HSPICE or HSPICE RF calculates the gate capacitors
and overlaps, from the IDS model for LEVEL 49 or 53. Simulation ignores
the CAPOP parameter; instead, use the CAPMOD model parameter, with a
reasonable value.
Guidelines for Choosing Accuracy Options
Use .OPTION ACCURATE for:
■
Analog or mixed signal circuits.
■
Circuits with long time constants, such as RC networks.
■
Circuits with ground bounce.
Use the default options (DVDT=4) for:
■
Digital CMOS.
■
CMOS cell characterization.
■
Circuits with fast moving edges (short rise and fall times).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
329
Chapter 9: Transient Analysis
Numerical Integration Algorithm Controls
For ideal delay elements, use one of the following:
■
ACCURATE.
■
DVDT=3.
■
DVDT=4. If the minimum pulse width of a signal is less than the minimum
ideal delay, set DELMAX to a value smaller than the minimum pulse width.
Numerical Integration Algorithm Controls
In HSPICE transient analysis, you can select one of three options to convert
differential terms into algebraic terms:
■
Gear
■
Backward-Euler
■
Trapezoidal
Gear algorithm:
.OPTION METHOD=GEAR
Backward-Euler:
.OPTION METHOD=GEAR MU=0
Trapezoidal algorithm (default):
.OPTION METHOD=TRAP
Each algorithm has advantages and disadvantages. Ideally, the trapezoidal is
the preferred algorithm overall, because of its highest accuracy level and lowest
simulation time.
However, selecting the appropriate algorithm for convergence is not always that
easy or ideal. Which algorithm you select, largely depends on the type of
circuit, and its associated behavior when you use different input stimuli.
Gear and Trapezoidal Algorithms
The algorithm that you select, automatically sets the timestep control algorithm.
In HSPICE, if you select the GEAR algorithm (including Backward-Euler), the
timestep control algorithm defaults to the truncation timestep algorithm.
However, if you select the trapezoidal algorithm, the DVDT algorithm is the
default. To change these HSPICE defaults, use the timestep control options.
330
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Numerical Integration Algorithm Controls
Figure 46
Time Domain Algorithm
Initialization.IC
NODESET
Iteration Solution
Converged
Reversal
Time Step Algorithm
Advancement
(tnew = told + Δt)
Time Step Unit Check
Timestep too
small error
Fail
Extrapolated Solution
for timepoint n
The trapezoidal algorithm can cause computational oscillation—that is,
oscillation that the algorithm itself causes, not oscillation from the circuit
design. This also produces an unusually long simulation time. If this occurs in
inductive circuits (such as switching regulators), use the GEAR algorithm.
If transient analysis fails to converge using .OPTION METHOD=TRAP and DVDT
timesteps (for example, due to trapezoidal oscillation), and HSPICE reports an
internal timestep too small error, HSPICE then starts the autoconvergence
process by default. This process sets .OPTION METHOD=GEAR and
LVLTIM=2, and uses the Local Truncation Error (LTE) timestep algorithm.
HSPICE then runs another transient analysis, to automatically obtain
convergent results.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
331
Chapter 9: Transient Analysis
Numerical Integration Algorithm Controls
To manually improve on autoconvergence results, or if autoconvergence fails to
converge, you can do either of the following:
■
Set .OPTION METHOD=GEAR in the netlist, and try to obtain convergent
results directly.
To improve accuracy or speed, you can adjust TSTEP in a .TRAN statement,
or in transient control options (such as RMAX, RELQ, CHGTOL, or TRTOL).
■
Set .OPTON METHOD=TRAP in the netlist, then manually adjust TSTEP and
the relevant control options (such as CSHUNT or GSHUNT).
Figure 47
Iteration Algorithm
Initial Guess
Element Evaluation
I.V.Q. Flux
Linearization of non-linear elements
Element Convergence Test
Gear or Trapezoidal
ABSI
RELI
ABSMOS
RELMOS
METHOD
MAXORD
GMIN
Assemble and Solve Matrix Equations
PIVOT
PIVREL
PIVTOL
ABSV
FAIL
Nodal Voltage Convergence Test
RELV
NEWTOL
Converged
332
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Numerical Integration Algorithm Controls (HSPICE RF)
Numerical Integration Algorithm Controls (HSPICE RF)
The numerical integration algorithm control in HSPICE RF is described in “RF
Numerical Integration Algorithm Control” in the HSPICE RF Manual.
Selecting Timestep Control Algorithms
In HSPICE or HSPICE RF, you can select one of three dynamic timestepcontrol algorithms:
■
Iteration Count Dynamic Timestep
■
Local Truncation Error Dynamic Timestep
■
DVDT Dynamic Timestep
Each algorithm uses a dynamically-changing timestep, which increases the
accuracy of simulation, and reduces the simulation time. To do this, simulation
varies the value of the timestep, over the transient analysis sweep, depending
on the stability of the output. Dynamic timestep algorithms increase the
timestep value when internal nodal voltages are stable, and decrease the
timestep value when nodal voltages change quickly.
Figure 48
Internal Variable Timestep
Changing Time Step - Dynamic
ΔtD-1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
ΔtD
333
Chapter 9: Transient Analysis
Selecting Timestep Control Algorithms
The LVLTIM option selects the timestep algorithm:
■
LVLTIM=0 selects the iteration count algorithm.
■
LVLTIM=1 selects the DVDT timestep algorithm, and the iteration count
algorithm. To control operation of the timestep control algorithm, set the
DVDT control option. For LVLTIM=1 and DVDT=0, 1, 2, or 3, the algorithm
does not use timestep reversal. For DVDT=4, the algorithm uses timestep
reversal.
For more information about the DVDT algorithm, see DVDT Dynamic
Timestep on page 335.
■
LVLTIM=2 selects the truncation timestep algorithm, and the iteration count
algorithm (with reversal).
■
LVLTIM=3 selects the DVDT timestep algorithm (with timestep reversal),
and the iteration count algorithm. For LVLTIM=3 and DVDT=0, 1, 2, 3, or 4,
the algorithm uses timestep reversal.
If HSPICE or HSPICE RF starts the autoconvergence process, it sets
LVLTIM=2.
Iteration Count Dynamic Timestep
The simplest dynamic timestep algorithm is the iteration count algorithm. The
control options that control this algorithm are .OPTION IMAX and .OPTION
IMIN.
Local Truncation Error Dynamic Timestep
The local truncation error (LTE) timestep algorithm uses a Taylor-series
approximation to calculate the next timestep for a transient analysis. This
algorithm uses the allowed LTE to calculate an internal timestep.
334
■
If the calculated timestep is smaller than the current timestep, HSPICE or
HSPICE RF sets back the timepoint (timestep reversal), and uses the
calculated timestep to increment the time.
■
If the calculated timestep is larger than the current timestep, then HSPICE
or HSPICE RF does not reverse the timestep. The next timepoint uses a
new timestep.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Selecting Timestep Control Algorithms
To select the LTE timestep algorithm, set LVLTIM=2 or METHOD=GEAR. The
control options available with the algorithm for local truncation error, are:
TRTOL (default=7)
CHGTOL (default=1e-15)
RELQ (default=0.01)
For some circuits (such as magnetic core circuits), GEAR and LTE provide
more accurate result than TRAP. You can use this method with circuits
containing inductors, diodes, BJTs (even Level 4 and above), MOSFETs, or
JFETs.
DVDT Dynamic Timestep
To select DVDT dynamic timestep algorithm, set the LVLTIM option to 1 or 3.
■
If you set LVLTIM=1, the DVDT algorithm does not use timestep reversal.
HSPICE or HSPICE RF saves the results for the current timepoint, and uses
a new timestep for the next timepoint.
■
If you set LVLTIM=3, the algorithm uses timestep reversal. If the results do
not converge at a specified iteration, HSPICE or HSPICE RF ignores the
results of the current timepoint, sets back the time by the old timestep, and
then uses a new timestep. Therefore, LVLTIM=3 is more accurate, and
more time-consuming, than LVLTIM=1.
This algorithm uses different tests, to decide whether to reverse the
timestep, depending on how you set the DVDT control option.
■
For DVDT=0, 1, 2, or 3, the decision is based on the SLOPETOL control
option.
■
For DVDT=4, the decision is based on how you set the SLOPETOL, RELVAR,
and ABSVAR control options.
The DVDT algorithm calculates the internal timestep, based on the rate of nodal
voltage changes.
■
For circuits with rapidly-changing nodal voltages, the DVDT algorithm uses
a small timestep.
■
For circuits with slowly-changing nodal voltages, the DVDT algorithm uses
larger timesteps.
The DVDT=4 setting selects a timestep control algorithm for non-linear node
voltages. If you set the LVLTIM option to either 1 or 3, then DVDT=4 also uses
timestep reversals. To measure non-linear node voltages, HSPICE or HSPICE
HSPICE® Simulation and Analysis User Guide
Y-2006.03
335
Chapter 9: Transient Analysis
Selecting Timestep Control Algorithms
RF measures changes in slopes of the voltages. If the change in slope is larger
than the SLOPETOL control setting, simulation reduces the timestep by the
factor set in the FT control option. The FT option defaults to 0.25.
HSPICE or HSPICE RF sets the SLOPETOL value to 0.75 for LVLTIM=1, and to
0.50 for LVLTIM=3. Reducing the value of SLOPETOL increases simulation
accuracy, but also increases simulation time.
■
For LVLTIM=1, SLOPETOL and FT control simulation accuracy.
■
For LVLTIM=3, the RELVAR and ABSVAR control options also affect the
timestep, and therefore affect the simulation accuracy.
Use .OPTION RELVAR and .OPTION ABSVAR with the DVDT option to
improve simulation time or accuracy. For faster simulation time, increase
RELVAR and ABSVAR (but this might decrease accuracy).
Note:
If you need backward compatibility, use these options. Setting .OPTION
DVDT=3 automatically sets all of these values.
LVLTIM=1 RMAX=2 SLOPETOL=0.5
FT=FS=0.25 BYPASS=0 BYTOL=0.050
Timestep Controls in HSPICE
The RMIN, RMAX, FS, FT, and DELMAX control options define the minimum and
maximum internal timestep for the DVDT dynamic timestep algorithm. If the
timestep is below the minimum, program execution stops. For example, if the
timestep becomes less than the minimum internal timestep (defined as
TSTEP*RMIN), HSPICE reports an internal timestep too small error.
Note:
TSTEP is the time increment set in the .TRAN statement. RMIN is the
minimum timestep coefficient. Default is 1e-9.
If you set .OPTION DELMAX, HSPICE uses DVDT=0. If you do not
specify .OPTION DELMAX, then HSPICE computes a DELMAX value. For
DVDT=0, 1, or 2, the maximum internal timestep is:
min[(TSTOP/50), DELMAX, (TSTEP*RMAX)]
The TSTOP time is the transient sweep range, as set in the .TRAN statement.
One exception is in the autospeedup process. When dealing with large nonlinear circuit with very big TSTOP or TSTEP values (for example, .TRAN 1n 1),
336
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Selecting Timestep Control Algorithms
HSPICE might activate autospeedup. This process automatically sets RMAX to
a bigger value, and sets the maximum internal timestep to:
min[(TSTOP/20),(TSTEP*RMAX)]
Set TRCON=-1 to disable autospeedup. You can then adjust TSTEP and RMAX,
to balance accuracy and speed.
In circuits with piecewise linear (PWL) transient sources, then .OPTION
SLOPETOL also affects the internal timestep. A PWL source, with a large
number of voltage or current segments, contributes a correspondingly-large
number of entries to the internal breakpoint table. The number of breakpoint
table entries contributes to the internal timestep control.
If the difference in the slope for consecutive segments of a PWL source, is less
than the SLOPETOL value, then HSPICE ignores the breakpoint table entry for
the point between the segments. For a PWL source, with a signal that changes
value slowly, ignoring its breakpoint table entries can help reduce the
simulation time. Data in the breakpoint table is a factor in the internal timestep
control, so setting a high SLOPETOL reduces the number of usable breakpoint
table entries, which reduces the simulation time.
Effect of TSTEP on Timestep Size Selection
HSPICE's timestep size selection is affected by:
■
voltage, current, and charge tolerances
■
value of the .TRAN statement TSTEP argument
■
value of the RMAX option
■
settings of the timestep control method options such as RUNLVL, LVLTIM,
and DVDT.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
337
Chapter 9: Transient Analysis
Fourier Analysis
The affect of TSTEP and RMAX depend on the timestep control method in use.
■
If RUNLVL=0, HSPICE never takes timesteps larger than TSTEP*RMAX. The
size of the timestep is controlled by voltage, current, and charge tolerances,
and LVLTIM/DVDT, but in any case, the step size is never allowed to exceed
TSTEP*RMAX.
■
If RUNLVL>0, HSPICE is allowed to take timesteps larger than
TSTEP*RMAX. The size of the timestep is controlled by voltage, current, and
charge tolerances. However, these tolerance values are affected by
TSTEP*RMAX, so that smaller TSTEP values do result in tighter tolerances
and therefore, smaller timesteps.
Compared with RUNLV=0, this tends to result in larger timesteps and faster
simulation speeds, especially in regions with flat or slowly varying
waveforms.
Timestep Controls in HSPICE RF
The timestemp controls in HSPICE RF are described in “RF Transient Analysis
Accuracy Control” in the HSPICE RF Manual.
Fourier Analysis
This section describes the Fourier and FFT Analysis flow for HSPICE.
338
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Fourier Analysis
Figure 49
Fourier and FFT Analysis
.FOUR Statement
Transient
Time-sweep
simulation
.FFT
.FOUR
Output Variables
Display Options
.FFT Statement
Transient
Output Variable
V
I
Time-sweep
simulation
.FFT
.FOUR
Display Option
P
Other
Window
Format
HSPICE provides two different Fourier analyses, but HSPICE RF does not
support either type of Fourier analysis:
■
.FOUR is the same as is available in SPICE 2G6: a standard, fixed-window
analysis tool. The .FOUR statement performs a Fourier analysis, as part of
the transient analysis.
■
.FFT is a much more flexible Fourier analysis tool. Use it for analysis tasks
that require more detail and precision.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
339
Chapter 9: Transient Analysis
Fourier Analysis
Accuracy and DELMAX
For better accuracy, set small values for .OPTION RMAX or .OPTION DELMAX.
For maximum accuracy, set .OPTION DELMAX to (period/500). For circuits with
very high resonance factors (high-Q circuits, such as crystal oscillators, tank
circuits, and active filters), set DELMAX to less than (period/500).
Fourier Equation
The total harmonic distortion is the square root of the sum of the squares, of
the second through ninth normalized harmonic, times 100, expressed as a
percent:
⎛ 9
⎞
1
⎜
2
-----⋅
THD =
R ⎟
R1 ⎜ ∑ m⎟
⎝m = 2 ⎠
1/2
⋅ 100%
This interpolation can result in various inaccuracies.
If the transient analysis runs at intervals longer than 1/(501*f), then the
frequency response of the interpolation dominates the power spectrum.
Furthermore, this interpolation does not derive an error range for the output.
The following equation calculates the Fourier coefficients:
9
g( t) =
9
∑
C m ⋅ cos ( mt ) +
m=0
∑
D m ⋅ sin ( mt )
m=0
The following equations calculate values for the preceding equation:
π
Cm
1
= --- ⋅
π
∫ g ( t ) ⋅ cos ( m ⋅ t ) ⋅dt
–π
π
Dm
1
= --- ⋅
π
∫ g ( t ) ⋅ sin ( m ⋅ t ) ⋅dt
–π
9
g( t) =
∑
m=0
340
9
C m ⋅ cos ( m ⋅ t ) +
∑
D m ⋅ sin ( m ⋅ t )
m=0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 9: Transient Analysis
Fourier Analysis
The following equations approximate the C and D values:
500
Cm =
2⋅π⋅m⋅n
-⎞
∑ g ( n ⋅ Δt ) ⋅ cos ⎛⎝ -------------------------501 ⎠
n=0
500
Dm =
2⋅π⋅m⋅n
-⎞
∑ g ( n ⋅ Δt ) ⋅ sin ⎛⎝ -------------------------501 ⎠
n=0
The following equations calculate the magnitude and phase:
R m = ( C m2 + D m2 ) 1 / 2
Cm
Φ m = arctan ⎛ -------⎞
⎝ D m⎠
Example 1
The following is input for an .OP, .TRAN, or .FOUR analysis. This example is
based on demonstration netlist four.sp, which is available in directory
$<installdir>/demo/hspice/apps:
CMOS INVERTER
*
M1 2 1 0 0 NMOS W=20U L=5U
M2 2 1 3 3 PMOS W=40U L=5U
VDD 3 0 5
VIN 1 0 SIN 2.5 2.5 20MEG
*
.MODEL NMOS NMOS LEVEL=3 CGDO=0.2N CGSO=0.2N CGB0=2N
.MODEL PMOS PMOS LEVEL=3 CGDO=0.2N CGSO=0.2N CGB0=2N
.OP
.TRAN 1N 500N
.FOUR 20MEG V(2)
.PRINT TRAN V(2) V(1)
.END
Example 2
******
cmos inverter
**** fourier analysis
tnom = 25.000 temp = 25.000 ****
fourier components of transient response v(2)
dc component=2.430D+00
harmonic
frequency fourier
normalized phase
normalized
no
(hz)
component
component (deg)
phase (deg)
1
20.0000x
3.0462
1.0000
176.5386
0.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
341
Chapter 9: Transient Analysis
Fourier Analysis
2
3
4
5
6
7
8
9
40.0000x
60.0000x
80.0000x
100.0000x
120.0000x
140.0000x
160.0000x
180.0000x
total harmonic
115.7006m
37.9817m -106.2672 -282.8057
753.0446m 247.2061m 170.7288
-5.8098
77.8910m
25.5697m -125.9511 -302.4897
296.5549m
97.3517m 164.5430
-11.9956
50.0994m
16.4464m -148.1115
-324.6501
125.2127m
41.1043m 157.7399
-18.7987
25.6916m
8.4339m 172.9579
-3.5807
47.7347m
15.6701m 154.1858
-22.3528
distortion=
27.3791
percent
Spectrum analysis represents a time-domain signal, within the frequency
domain. It most commonly uses the Fourier transform. A Discrete Fourier
Transform (DFT) uses sequences of time values to determine the frequency
content of analog signals, in circuit simulation.
The Fast Fourier Transform (FFT) calculates the DFT, which Synopsys HSPICE
uses for spectrum analysis. The .FFT statement uses the internal time point
values.
By default, .FFT uses a second-order interpolation to obtain waveform
samples, based on the number of points that you specify.
You can use windowing functions to reduce the effects of waveform truncation
on the spectral content. You can also use the .FFT command to specify:
342
■
output format
■
frequency
■
number of harmonics
■
total harmonic distortion (THD)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
10
10
AC Sweep and Small Signal Analysis
Describes how to perform AC sweep and small signal analysis.
This chapter covers AC small signal analysis, AC analysis of an RC network,
and other AC analysis statements. For information on output variables, see AC
Analysis Output Variables on page 260.
For descriptions of individual HSPICE commands referenced in this chapter,
see the HSPICE Command Reference.
Using the .AC Statement
You can use the .AC statement for the following applications:
■
Single/double sweeps
■
Sweeps using parameters
■
.AC analysis optimization
■
Random/Monte Carlo anlayses
For .AC command syntax and examples, see the .AC command in the HSPICE
Command Reference.
.AC Control Options
You can use the following .AC control options when performing an AC analysis:
ABSH
ACOUT
DI
MAXAMP
RELH
UNWRAP
HSPICE® Simulation and Analysis User Guide
Y-2006.03
343
Chapter 10: AC Sweep and Small Signal Analysis
AC Small Signal Analysis
For syntax descriptions for these options, see the “Netlist Control Options”
chapter in the HSPICE Command Reference.
AC Small Signal Analysis
AC small signal analysis in HSPICE or HSPICE RF computes AC output
variables as a function of frequency (see Figure 50 on page 344). HSPICE or
HSPICE RF first solves for the DC operating point conditions. It then uses
these conditions to develop linear, small-signal models for all non-linear
devices in the circuit.
Figure 50
AC Small Signal Analysis Flow
Simulation Experiment
DC
Transient
Other AC analysis
statements
AC
AC small-signal
simulation
.NOISE
.DISTO
.SAMPLE
.NETWORK
.OPTION:
Method
DC options, to solve
operating-point
ABSH
ACOUT
DI
MAXAMP
RELH
UNWRAP
In HSPICE or HSPICE RF, the output of AC Analysis includes voltages and
currents.
344
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 10: AC Sweep and Small Signal Analysis
AC Small Signal Analysis
HSPICE or HSPICE RF converts capacitor and inductor values to their
corresponding admittances:
y C = jωC for capacitors
1
y L = --------for inductors
jωL
Resistors can have different DC and AC values. If you specify AC=<value> in
a resistor statement, HSPICE or HSPICE RF uses the DC value of resistance
to calculate the operating point, but uses the AC resistance value in the AC
analysis. When you analyze operational amplifiers, HSPICE or HSPICE RF
uses a low value for the feedback resistance to compute the operating point for
the unity gain configuration. You can then use a very large value for the AC
resistance in AC analysis of the open loop configuration.
AC analysis of bipolar transistors is based on the small-signal equivalent circuit,
as described in the HSPICE Elements and Device Models Manual. MOSFET
AC-equivalent circuit models are described in the HSPICE Elements and
Device Models Manual.
The AC analysis statement can sweep values for:
■
Frequency.
■
Element.
■
Temperature.
■
Model parameter (HSPICE and HSPICE RF).
■
Randomized (Monte Carlo) distribution (HSPICE only; not supported in
HSPICE RF).
■
Optimization and AC analysis (HSPICE or HSPICE RF).
Additionally, as part of the small-signal analysis tools, HSPICE or HSPICE RF
provides:
■
Noise analysis.
■
Distortion analysis.
■
Network analysis.
■
Sampling noise.
You can use the .AC statement in several different formats, depending on the
application. You can also use the .AC statement to perform data-driven
analysis in HSPICE, but not in HSPICE RF.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
345
Chapter 10: AC Sweep and Small Signal Analysis
AC Analysis of an RC Network
AC Analysis of an RC Network
Figure 51 on page 346 shows a simple RC network with a DC and AC source
applied. The circuit consists of:
■
Two resistors, R1 and R2.
■
Capacitor C1.
■
Voltage source V1.
■
Node 1 is the connection between the source positive terminal and R1.
■
Node 2 is where R1, R2, and C1 are connected.
■
HSPICE ground is always node 0.
Figure 51
RC Network Circuit
1
R1
1k
V1
10 VDC
1VAC
2
+
_
R2
1k
C1
0.001 mF
0
The netlist for this RC network is based on demonstration netlist quickAC.sp,
which is available in directory $<installdir>/demo/hspice/apps:
A SIMPLE AC RUN
.OPTION LIST NODE POST
.OP
.AC DEC 10 1K 1MEG
.PRINT AC V(1) V(2) I(R2) I(C1)
V1 1 0 10 AC 1
R1 1 2 1K
R2 2 0 1K
C1 2 0 .001U
.END
346
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 10: AC Sweep and Small Signal Analysis
AC Analysis of an RC Network
Follow the procedure below to perform AC analysis for an RC network circuit.
1. Type the above netlist into a file named quickAC.sp.
2. To run a HSPICE analysis, type:
hspice quickAC.sp > quickAC.lis
For HSPICE RF, type:
hspicext quickAC.sp > quickAC.lis
When the run finishes, HSPICE displays:
>info:
***** hspice job concluded
This is followed by a line that shows the amount of real time, user time, and
system time needed for the analysis.
Your run directory includes the following new files:
•
quickAC.ac0
•
quickAC.ic0
•
quickAC.lis
•
quickAC.st0
3. Use an editor to view the .lis and .st0 files to examine the simulation results
and status.
4. Run AvanWaves and open the .sp file.
5. To view the waveform, select the quickAC.ac0 file from the Results Browser
window.
6. Display the voltage at node 2 by using a log scale on the x-axis.
Figure 52 on page 348 shows the waveform that HSPICE or HSPICE RF
produces if you sweep the response of node 2, as you vary the frequency of the
input from 1 kHz to 1 MHz.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
347
Chapter 10: AC Sweep and Small Signal Analysis
Other AC Analysis Statements
Figure 52
RC Network Node 2 Frequency Response
A simple AC run
04/14/2003 16:52:48
500.0m
quickAC.ac
2*m
volt maglin
450.0m
400.0m
350.0m
300.0m
250.0m
200.0m
151.657m
1.0k
10.0k
100.k
1.0x
hertz (log)
As you sweep the input from 1 kHz to 1 MHz, the quickAC.lis file displays:
■
Input netlist.
■
Details about the elements and topology.
■
Operating point information.
■
Table of requested data.
The quickAC.ic0 file contains information about DC operating point conditions.
The quickAC.st0 file contains information about the simulation run status.
To use the operating point conditions for subsequent simulation runs, execute
the .LOAD statement (HSPICE only; HSPICE RF does not support the .LOAD
statement).
Other AC Analysis Statements
The following sections describe the commands you can use to perform other
types of AC analyses:
■
Using .DISTO for Small-Signal Distortion Analysis on page 349
■
Using .NOISE for Small-Signal Noise Analysis on page 349
■
Using .SAMPLE for Noise Folding Analysis on page 350
Use the .NOISE and .AC statements to control the noise analysis of the circuit.
348
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 10: AC Sweep and Small Signal Analysis
Other AC Analysis Statements
Using .DISTO for Small-Signal Distortion Analysis
The .DISTO statement computes the distortion characteristics of the circuit in
an AC small-signal, sinusoidal, steady-state analysis. HSPICE computes and
reports five distortion measures at the specified load resistor. The analysis is
performed assuming that one or two signal frequencies are imposed at the
input. The first frequency, F1 (used to calculate harmonic distortion), is the
nominal analysis frequency set by the .AC statement frequency sweep. The
optional second input frequency, F2 (used to calculate intermodulation
distortion), is set implicitly by specifying the skw2 parameter, which is the ratio
F2/F1.
For command syntax and examples, see the .DISTO command in the HSPICE
Command Reference.
Using .NOISE for Small-Signal Noise Analysis
Noise calculations in HSPICE or HSPICE RF are based on complex AC nodal
voltages, which in turn are based on the DC operating point. For descriptions of
noise models for each device type, see the HSPICE Elements and Device
Models Manual. Each noise source does not statistically correlate to other
noise sources in the circuit; the HSPICE or HSPICE RF simulator calculates
each noise source independently. The total output noise voltage is the RMS
sum of the individual noise contributions:
N
onoise =
∑
2
Zk i nk
2
k=0
Where,
onoise is the total output noise (HSPICE or HSPICE RF).
ink is the normal current source due to thermal, shot, or other noise.
Zk is the equivalent transimpedance between each noise current source and
output.
N is the number of noise sources associated with all circuit elements.
The input noise (inoise) voltage is the total output noise divided by the gain or
transfer function of the circuit. HSPICE or HSPICE RF prints the contribution of
each noise generator in the circuit for each inter frequency point. The simulator
HSPICE® Simulation and Analysis User Guide
Y-2006.03
349
Chapter 10: AC Sweep and Small Signal Analysis
Other AC Analysis Statements
also normalizes the output and input noise levels relative to the square root of
the noise bandwidth. The units are volts/Hz1/2 or amps/Hz1/2.
To simulate flicker noise sources in the noise analysis, include values for the KF
and AF parameters on the appropriate device model statements. Use
the .PRINT or .PLOT statement to print or plot output noise, and the
equivalent input noise.
If you specify more than one .NOISE statement in a single simulation, HSPICE
or HSPICE RF runs only the last statement.
Table 46
.NOISE Measurements Available for MOSFETs
.ac
.lis
Unit
Description
nd
rd
2
V
------Hz
Output thermal noise due to drain resistor
ns
rs
2
V
------Hz
Output thermal noise due to source resistor
ni
id
2
V
------Hz
Output channel thermal noise
nf
fn
2
V
------Hz
Output flicker noise
ntg
total
2
V
------Hz
Total output noise:
TOT=RD + RS + ID + FN
Using .SAMPLE for Noise Folding Analysis
For data acquisition of analog signals, data sampling noise often needs to be
analyzed. This is accomplished with the .SAMPLE statement used in
conjunction with the .NOISE and .AC statements. The SAMPLE analysis
performs a simple noise folding analysis at the output node.
For the syntax and description of the .SAMPLE statement, see the .SAMPLE
command in the HSPICE Command Reference.
350
HSPICE® Simulation and Analysis User Guide
Y-2006.03
11
11
Linear Network Parameter Analysis
Describes how to perform an AC sweep to extract small-signal linear network
parameters.
The chapter covers .LIN analysis, RF measurements from .LIN, extracting
mixed-mode S (scattering) parameters, and .NET parameter analysis.
For descriptions of individual HSPICE commands referenced in this chapter,
see the HSPICE Command Reference.
.LIN Analysis
The .LIN command extracts noise and linear transfer parameters for a general
multi-port network.
When used with the .AC command, .LIN makes available a broad set of
linear port-wise measurements:
■
Multi-port scattering [S] parameters
■
Noise parameters
■
Stability factors
■
Gain factors
■
Matching coefficients
The .LIN analysis is similar to basic small-signal, swept-frequency .AC
analysis, but it also automatically calculates a series of noise and small-signal
transfer parameters between the terminals identified using port (P) elements.
HSPICE can output the result of group delay extraction and two-port noise
analysis to either a .sc* file, a Touchstone file, or a CITIfile.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
351
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
The .PRINT/.PROBE/.MEAS output syntax for .LIN supports H (hybrid)
parameters and S/Y/Z/H group delay.
Figure 53
Basic Circuit in .LIN Analysis
I1
Z01
P1
I2
+
V1
-
Circuit
under
test
+
V2
P2
Z02
-
Identifying Ports with the Port Element
The .LIN command computes the S (scattering), Y (admittance), and Z
(impedance) parameters directly based on the location of the port (P) elements
in your circuit, and the specified values for their reference impedances.
The port element identifies the ports used in .LIN analysis. Each port element
requires a unique port number. If your design uses N port elements, your netlist
must contain the sequential set of port numbers 1 through N (for example, in a
design containing 512 ports, you must number each port sequentially 1 to 512).
Each port has an associated system impedance, z0. If you do not explicitly
specify the system impedance, the default is 50 ohms.
The port element behaves as either a noiseless impedance or a voltage source
in series with the port impedance for all other analyses (DC, AC, or TRAN).
■
You can use this element as a pure terminating resistance or as a voltage or
power source.
■
You can use the RDC, RAC, RHB, RHBAC, and rtran values to override the port
impedance value for a particular analysis.
Syntax
Pxxx p n port=portnumber
+ $ **** Voltage or Power Information ********
+ <DC mag> <AC <mag <phase>>> <HBAC <mag <phase>>>
+ <HB <mag <phase <harm <tone <modharm <modtone>>>>>>>
+ <transient_waveform> <TRANFORHB=[0|1]>
+ <DCOPEN=[0|1]>
+ $ **** Source Impedance Information ********
352
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
+
+
+
+
<Z0=val> <RDC=val> <RAC=val>
<RHBAC=val> <RHB=val> <RTRAN=val>
$ **** Power Switch ********
<power=[0|1|2|W|dbm]>
Parameter
Description
port=portnumber
The port number. Numbered sequentially beginning
with 1 with no shared port numbers.
<DC mag>
DC voltage or power source value.
<AC <mag <phase>>>
AC voltage or power source value.
<HBAC <mag <phase>>>
(HSPICE RF) HBAC voltage or power source value.
<HB <mag <phase <harm
<tone <modharm
<modtone>>>>>>>
(HSPICE RF) HB voltage, current, or power source
value. Multiple HB specifications with different harm,
tone, modharm, and modtone values are allowed.
■
■
HSPICE® Simulation and Analysis User Guide
Y-2006.03
phase is in degrees
harm and tone are indices corresponding to the
tones specified in the .HB statement. Indexing sta4 r(m)-2.1(0 Tw(to(
353
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Parameter
Description
<TRANFORHB=[0|1]>
■
0 (default): The transient description is ignored if an
HB value is given or a DC value is given. If no DC or
HB value is given and TRANFORHB=0, then HB
analysis treats the source as a DC source, and the
DC source value is the time=0 value.
■
1: HB analysis uses the transient description if its
value is VMRF, SIN, PULSE, PWL, or LFSR. If the
type is a non-repeating PWL source, then the
time=infinity value is used as a DC analysis source
value. For example, the following statement is treated
as a DC source with value=1 for HB analysis:
v1 1 0 PWL (0 0 1n 1 1u 1)
+ TRANFORHB=1
In contrast, the following statement is a 0V DC
source:
v1 1 0 PWL (0 0 1n 1 1u 1)
+ TRANFORHB=0
The following statement is treated as a periodic
source with a 1us period that uses PWL values:
v1 1 0 PWL (0 0 1n 1 0.999u 1 1u 0) R
+ TRANFORHB=1
To override the global TRANFORHB option, explicitly
set TRANFORHB for a voltage or current source.
DCOPEN
Switch for open DC connection when DC mag is not set.
■
■
<z0=val>
0 (default): P element behaves as an impedance
termination.
1 : P element is considered an open circuit in DC
operating point analysis. DCOPEN=1 is mainly used
in .LIN analysis so the P element will not affect the
self-biasing device under test by opening the
termination at the operating point.
(LIN analysis) System impedance used when
converting to a power source, inserted in series with the
voltage source. Currently, this only supports real
impedance.
■
When power=0, z0 defaults to 0.
When power=1, z0 defaults to 50 ohms.
You can also enter z0=val.
■
354
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Parameter
Description
<RDC=val>
(DC analysis) Series resistance (overrides z0).
<RAC=val>
(AC analysis) Series resistance (overrides z0).
<RHBAC=val>
(HSPICE RF HBAC analysis) Series resistance
(overrides z0).
<RHB=val>
(HSPICE RF HB analysis) Series resistance (overrides
z0).
<RTRAN=val>
(Transient analysis) Series resistance (overrides z0).
<power=[0 | 1 | 2 | W | dbm]> (HSPICE RF) power switch
■
When 0 (default), element treated as a voltage or
current source.
■
When 1 or W, element treated as a power source,
realized as a voltage source with a series
impedance. In this case, the source value is
interpreted as RMS available power in units of Watts.
■
When 2 or dbm, element treated as a power source
in series with the port imedance. Values are in dbms.
You can use this parameter for Transient analysis if the
power source is either DC or SIN.
Example
For example, the following port element specifications identify a 2-port network
with 50-Ohm reference impedances between the "in" and "out" nodes.
P1 in gnd port=1 z0=50
P2 out gnd port=2 z0=50
Computing scattering parameters requires z0 reference impedance values.
The order of the port parameters (in the P Element) determines the order of the
S, Y, and Z parameters. Unlike the .NET command, .LIN does not require you
to insert additional sources into the circuit. To calculate the requested transfer
parameters, HSPICE automatically inserts these sources as needed at the port
terminals. You can define an unlimited number of ports.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
355
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Using the P (Port) Element for Mixed-Mode Measurement
You can use a port element with three terminals as the port element for
measuring the mixed mode S parameters. Except for the number of external
terminals, the syntax of the port element remains the same. The .LIN analysis
function internally sets the necessary drive mode (common/differential) of
these mixed mode port elements. For analyses other than the .LIN analysis
(such as DC, AC, TRAN, and so on), the mixed-mode P Element acts as a
differential driver that drives positive nodes with half of their specified voltage
and the negative nodes with a negated half of the specified voltage. Figure 54
shows the block diagram of the mixed mode port element.
Figure 54
Mixed Mode Port Element
P1 (port element)
n1+
Zo
Zo
V+
Vn2-
n1_ref
P1 n1+ n1- n1_ref Zo=50
The port element can also be used as a signal source with a built in reference
impedance. For further information on its use as a signal source, see Chapter
5, Sources and Stimuli.
.LIN Input 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]>
356
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
For argument descriptions, see the .LIN command in the HSPICE Command
Reference.
.LIN Output Syntax
This section describes the syntax for the .PRINT and .PROBE statements
used for LIN analysis.
.PRINT and .PROBE Statements
.PRINT AC <Xmn | Xmn LINPARAM(TYPE) | X(m,n) |
+ X(m,n) LINPARAM(TYPE)> <Hmn | Hmn(TYPE) |
+ H(m,n) | H(m,n)(TYPE)>
.PROBE AC <Xmn | Xmn LINPARAM(TYPE) | X(m,n) |
+ X(m,n) LINPARAM(TYPE)> <Hmn | Hmn(TYPE) |
+ H(m,n) | H(m,n)(TYPE)>
Argument
Description
Xmn, X(m,n) One of these parameter types:
■
S (scattering parameters)
Y (admittance parameters)
■
Z (impedance parameters)
■
H (hybrid parameters)
mn refers to a pair of port numbers, where m can be 1 or 2, and n can
be 1 or 2.
■
Hmn,
H(m,n)
Complex hybrid (H-) parameters.
mn refers to a pair of port numbers, where m can be 1 or 2, and n can
be 1 or 2.
If m,n=0 or m,n>2, HSPICE issues a warning and ignores the output
request.
■
To calculate a one-port H parameter, you must specify at least one
port (P) element.
■
To calculate a two-port H parameter, you must specify two or more
port (P) elements.
For additional information, see Hybrid Parameter Calculations on
page 359.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
357
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Argument
Description
LINPARAM
Two-port noise parameters:
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
■
358
NFMIN (noise figure minimum)
NF (Noise figure)
VN2 (Equivalent input noise voltage squared
IN2 (Equivalent input noise current squared)
RHON (Correlation coefficient between input noise voltage and input
noise current)
RN (Noise equivalent resistance)
GN (Noise equivalent conductance)
ZCOR (Noise correlation impedance)
YCOR (Noise correlation admittance)
ZOPT (Optimum source impedance for noise)
YOPT (Optimum source admittance for noise)
GAMMA_OPT (source reflection coefficient that achieves the
minimum noise figure)
ZOPT (source impedance that achieves minimum noise)
RN (noise equivalent resistance)
K_STABILITY_FACTOR (Rollett stability factor)
MU_STABILITY_FACTOR (Edwards & Sinsky stability factor)
G_MAX (maximum available/operating power gain)
G_MSG (Maximum stable gain)
G_TUMAX (Maximum unilateral transducer power gain)
G_U (Unilateral power gain)
G_MAX_GAMMA1 (source reflection coefficient that achieves
maximum available power gain)
G_MAX_GAMMA2 (load reflection coefficient that achieves
maximum operating power gain)
G_MAX_Z1=Source impedance needed to realize G_MAX
(complex, Ohms)
G_MAX_Z2=Load impedance needed to realize G_MAX (complex,
Ohms)
G_MAX_Y1=Source admittance needed to realize G_MAX
(complex, Siemens)
G_MAX_Y2=Load admittance needed to realize G_MAX (complex,
Siemens)
G_AS (associate gain—maximum gain at the minimum noise figure)
VSWR(n) (voltage standing-wave ratio at the n port)
GD (group delay from port=1 to port=2)
G_MSG (maximum stable gain)
G_TUMAX (maximum unilateral transducer power gain)
G_U (unilateral power gain)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Argument
Description
TYPE
Data type definitions:
■
■
■
■
■
■
R=Real
I=Imaginary
M=Magnitude
P=PD=Phase in degrees
PR=Phase in radians
DB=decibels
Examples
.print AC S11 S21(DB) S(2,3)(D) S(2,1)(I)
.print AC NFMIN GAMMA_OPT G_AS
.probe AC RN G_MAX ZOPT Y(3,1)(M) Y31(P)
Hybrid Parameter Calculations
The hybrid parameters are transformed from S-parameters:
■
For a one-port circuit, the calculation is:
( 1 + S 11 )
H 11 = Z 01 --------------------( 1 – S 11 )
■
For a two-port circuit, the calculation is:
( 1 + S 11 ) ( 1 + S n ) – S 12 S 21
H 11 = Z 01 --------------------------------------------------------------( 1 – S 11 ) ( 1 + S n ) + S 12 S 21
H 12 =
2S 12
Z 02
-------- -----------------------------------------------------------------Z 01 ( 1 – S 11 ) ( 1 + S 22 ) + S 12 S 21
H 21 =
– S 21
Z 02
-------- -----------------------------------------------------------------Z 01 ( 1 – S 11 ) ( 1 + S 22 ) + S 12 S 21
1 ( 1 – S 11 ) ( 1 – S 22 ) – S 12 S 21
H 22 = -------- -----------------------------------------------------------------Z 02 ( 1 – S 11 ) ( 1 + S 22 ) + S 12 S 21
For networks with more than two ports when computing the 1,2 H index
parameters, HSPICE assumes that ports numbered 3 and above terminate in
their port reference impedance (z0). The above two-port calculations therefore
remain appropriate, because S11, S12, S21, and S22 remain valid, and
simulation can ignore higher order S-parameters.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
359
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Multi-Port Scattering (S) Parameters
S-parameters represent the ratio of incident and scattered (or forward and
reflected) normalized voltage waves. Figure 55 shows a two-port network.
Figure 55
Two-Port Network
I1
Port=1
Z01
I2
+
V1
Two-Port
Network
+
V2
-
Z02
Port=2
-
The following equations define the incident (forward) waves for this two-port
network:
v 1 + Z 01 I 1
a 1 = ----------------------2 ⋅ Z 01
v 2 + Z 02 I 2
a 2 = ----------------------2 ⋅ Z 02
The following equations define the scattered (reflected) waves for this two-port
network:
v 1 – Z 01 I 1
b 1 = ----------------------2 ⋅ Z 01
v 2 – Z 02 I 2
b 2 = ----------------------2 ⋅ Z 02
The following equations define the S parameters:
b
S 11 = ----1a1 a2 = 0
b
S 12 = ----1a2 a1 = 0
b
S 21 = ----2a1 a2 = 0
b
S 22 = ----2a2 a1 = 0
Each S-parameter is a complex number, which can represent gain, isolation, or
a reflection coefficient.
Example
The following examples show how you can represent a gain, isolation, or
reflection coefficient:
.PRINT AC S11(DB) $ Input return loss
.PRINT AC S21(DB) $ Gain
360
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
.PRINT AC S12(DB) $ Isolation
.PRINT AC S22(DB) $ Output return loss
Two-Port Transfer and Noise Calculations
Two-port noise analysis is a linear AC noise analysis method that determines
the noise figure of a linear two-port for an arbitrary source impedance.
Several output parameter measurements are specific to two-port
networks. .LIN analysis supports two-port calculations for 3 or more ports if
port=1 is the input and port=2 the output. All other ports terminate in their
characteristic impedance. This is equivalent to operating on the two-port [S]
sub-matrix extracted from the multi-port [S] matrix. This occurs for both signal
and noise calculations. A warning appears if N>2 and you specified two-port
quantities.
Noise and signal port-wise calculations do not require that port elements use a
ground reference. You can therefore measure fully-differential circuits.
.LIN generates a set of noise parameters. The analysis assumes a noise
model consisting of:
■
A shunt current noise source, called In, at the input of a noiseless two-port
linear network.
■
A series voltage noise source, called Vn, at the input of a noiseless two-port
linear network.
■
A source with impedance, called Zs, that drives this two-port network.
■
The two-port network drives a noiseless load, called Zl.
Equivalent Input Noise Voltage and Current
For each analysis frequency, HSPICE computes a noise equivalent circuit for a
linear two-port. The noise equivalent circuit calculation results in an equivalent
noise voltage and current, and their correlation coefficient.
■
VN2: Equivalent input noise voltage squared (Real, V2).
■
IN2: Equivalent input noise current squared (Real, A2).
■
RHON: Correlation coefficient between the input noise voltage and the input
noise current (complex, unitless).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
361
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Equivalent Noise Resistance and Conductance
These measurements are the equivalent resistance and conductance, which
generate the equivalent noise voltage and current values at a temperature of
T=290K in a 1Hz bandwidth.
■
RN: Noise equivalent resistance (Real, Ohms)
■
GN: Noise equivalent conductance (Real, Siemens)
Noise Correlation Impedance and Admittance
These measurements represent the equivalent impedance and admittance that
you can insert at the input of the noise equivalent circuit to account for the
correlation between the equivalent noise voltage and the current values.
■
ZCOR: Noise correlation impedance (Complex, Ohms)
■
YCOR: Noise correlation admittance (Complex, Siemens)
Optimum Matching for Noise
These measurements represent the optimum impedance, admittance, and
reflection coefficient value that result in the best noise performance (minimum
noise figure).
■
ZOPT: Optimum source impedance for noise (Complex, Ohms)
■
YOPT: Optimum source admittance for noise (Complex, Siemens)
■
GAMMA_OPT: Optimum source reflection coefficient (Complex, unitless)
Because ZOPT and YOPT can commonly take on infinite values when
computing optimum noise conditions, calculations for optimum noise loading
reflect the GAMMA_OPT coefficient.
Noise Figure and Minimum Noise Figure
Noise figure represents the ratio of the SNR (signal to noise ratio) at the input
to the SNR at the output. You can set the input source impedance to ZOPT to
obtain the minimum noise figure.
362
■
NFMIN: Minimum noise figure (source at ZOPT) (real, unitless, power ratio)
■
NF: Noise figure (value obtained with source impedance at Zc[1]) (real,
unitless, power ratio)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Associated Gain
This measurement assumes that the input impedance matches the minimum
noise figure, and the output matches the maximum gain.
G_AS is the associated gain—maximum power gain at NFMIN (real, power
ratio)
Output Format for Group Delay in .sc* Files
All of the S/Y/Z/H parameters support a group delay calculation. The output
syntax of .PRINT and .PROBE statement for group delay is:
Xmn(T) | Xmn(TD) | X(m,n)(T) | X(m,n)(TD)
■
X=S, Y, Z, or H
■
m, n=port number (1 or 2 for H parameter)
The output of group delay matrices in .sc* files lets HSPICE directly read back
the group delay information, the tabulated data uses the regular HSPICE model
syntax with the SP keyword:
*| group delay parameters
.MODEL SMODEL_GD SP N=2 SPACING=POI INTERPOLATION=LINEAR
+ MATRIX=NONSYMMETRIC VALTYPE=REAL
+ DATA=3
+
1e+08
+
0
5e-09
+
5e-09
0
+
{...data...}
model name is the model name of the S parameters, plus _GD.
GROUPDELAY=[0|1] in the top line indicates group delay data:
*| N=2 DATA=3 NOISE=0 GROUPDELAY=1
*| NumOfBlock=1 NumOfParam=0
Output Format for Two-Port Noise Parameters in .sc* Files
Output of two-port noise parameter data in .sc* files shows the tabulated data
with the following quantities in the following order:
*| 2-port noise parameters
*|
frequency Fmin[dB] GammaOpt(M) GammaOpt(P) RN/Z0
*|
{...data...}
HSPICE® Simulation and Analysis User Guide
Y-2006.03
363
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
In this syntax:
■
Fmin[dB]=minimum noise figure (dB).
■
GammaOpt(M)=magnitude of the reflection coefficient needed to realize
Fmin.
■
GammaOpt(P)=phase (degrees) of the reflection coefficient needed to
realize Fmin.
■
RN/Z0=normalized noise resistance.
Both GammaOpt and RN/Z0 values are normalized with respect to the
characteristic impedance of the port=1 element (that is, Z01).
Noise Parameters
You can use the .LIN analysis to compute the equivalent two-port noise
parameters for a network. The noisecalc=1 option automatically calculates
the following equivalent circuit values.
Figure 56
Noise Equivalent Circuit
Vn
+In
Port=1
Two-Port
Network
Port=2
■
Vn is the equivalent input-referred noise voltage source.
■
In is the equivalent input-referred noise current source.
■
InVn is their correlation.
HSPICE can output the result of .LIN noise analysis to a .sc*, Touchstone, or
CITIfile.
HSPICE noise analysis also makes the following measurements available:
Vn 2
R n = ---------4kT
364
In 2
G n = --------4kT
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
I n∗ V n
Z cor = ------------= R cor + jX cor
2
In
⎛
R
2⎞
F min = 1 + 2G n ⎜ R cor + ------n – ( X cor ) ⎟
Gn
⎝
⎠
Z opt =
R
2
------n – ( R cor ) – jX cor
Gn
Z opt – Z 0
γI opt = --------------------Z opt + Z 0
Hybrid (H) Parameters
.LIN analysis can calculate the complex two-port H (hybrid) parameter of a
multi-terminal network.
The H parameters of a two-port network relate the voltages and currents at
input and output ports:
V1 = h11 ⋅ I1 + h12 ⋅ V2
I2 = h21 ⋅ I1 + h22 ⋅ V2
In the preceding equations:
■
H = h11 h12 Hybrid matrix
h21 h22
■
V1=Voltage at input port
■
I2=Current at output port
■
V2=Voltage at output port
■
I1=Current at input port
You can add the hybrid H parameter matrixes of two networks to describe
networks that are in series at their input and in parallel at their output.
.LIN can calculate H parameters based on the scattering parameters of the
networks. .LIN analysis can extract one-port and two-port network H
parameters. For networks with more than two ports, .LIN assumes that the
ports numbered 3 and above terminate in their port characteristic impedance
(Zc[i], i>2).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
365
Chapter 11: Linear Network Parameter Analysis
.LIN Analysis
Group Delay
Group delay measures the transit time of a signal through a network versus
frequency. It reduces the linear portion of the phase response to a constant
value, and transforms the deviations from linear phase into deviations from
constant group delay (which causes phase distortion in communications
systems). The average delay represents the average signal transit time through
a network system.
HSPICE can output the result of .LIN group delay measurement to a .sc*,
Touchstone, or CITIfile.
Group delay is a function of frequency:
d ( phase )
gd ( w ) = –-------------------------d(w)
Where,
■
gd=Group delay at the f frequency, 2πf = w
■
phase=phase response at the f frequency
■
w=radians frequency
All complex S, Y, Z, and H parameters support a group delay calculation.
Syntax
Xmn(T) | Xmn(TD) | X(m,n)(T) | X(m,n)(TD)
X=S, Y, Z, or H (parameters)
m,n=port number (1 or 2 for H-parameters)
The results of the group delay calculation are scalar real numbers in units of
seconds. For .LIN, group delay values are a function of frequency. The
calculation is:
r ij = |r ij |e
jf ij ( w )
Differentiating the complex logarithm with respect to omega results in:
1 dr
1 d|r ij | -----df
----- -------ij- = -------- ----------+j r ij dw |r ij | dw
dw
366
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
The group delay is the negative derivative of the phase. Simulation can
compute it from the imaginary component of the derivative w.r.t. frequency of
the measurement:
dr
r ij dw
1 -------ijdf- = – Im ---τ ( w ) = – -----dw
RF Measurements From .LIN
In addition to S, Y, Z, and H parameters, a LIN analysis can include the output
measurements in the following sections.
Impedance Characterizations
■
VSWR(i)=Voltage standing wave ratio at port i (real, unit-less)
■
ZIN(i)=Input impedance at port i (complex, Ohms)
■
YIN(i)=Input admittance at port i (complex, Siemens)
Stability Measurements
■
K_STABILITY_FACTOR=Rollett stability factor (real, unit-less)
■
MU_STABILITY_FACTOR=Edwards & Sinsky stability factor (real, unit-less)
Gain Measurements
■
G_MAX=Maximum available/operating power gain (real, power ratio)
■
G_MSG=Maximum stable gain (real, power ratio)
■
G_TUMAX=Maximum unilateral transducer power gain (real, power ratio)
■
G_U=Unilateral power gain (real, power ratio)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
367
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
Matching for Optimal Gain
■
G_MAX_GAMMA1=Source reflection coefficient needed to realize G_MAX
(complex, unit-less)
■
G_MAX_GAMMA2=Load reflection coefficient needed to realize G_MAX
(complex, unit-less)
■
G_MAX_Z1=Source impedance needed to realize G_MAX (complex, Ohms)
■
G_MAX_Z2=Load impedance needed to realize G_MAX (complex, Ohms)
■
G_MAX_Y1=Source admittance needed to realize G_MAX (complex,
Siemens)
■
G_MAX_Y2=Load admittance needed to realize G_MAX (complex, Siemens)
Noise Measurements
368
■
VN2=Equivalent input noise voltage squared (real, V2)
■
IN2=Equivalent input noise current squared (real, A2)
■
RHON=Correlation coefficient between input noise voltage and input noise
current (complex, unit-less)
■
RN=Noise equivalent resistance (real, Ohms)
■
GN=Noise equivalent conductance (real, Siemens)
■
ZCOR=Noise correlation impedance (complex, Ohms)
■
YCOR=Noise correlation admittance (complex, Siemens)
■
ZOPT=Optimum source impedance for noise (complex, Ohms)
■
YOPT=Optimum source admittance for noise (complex, Siemens)
■
GAMMA_OPT=Optimum source reflection coefficient (complex, unit-less)
■
NFMIN=Noise figure minimum (source at Zopt) (real, unit-less power ratio)
■
NF=Noise figure (value obtained with source impedance at Z01) (real, unitless power ratio)
■
G_AS=Associated gain -- maximum power gain at NFMIN (real, power ratio)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
Two-Port Transfer and Noise Measurements
Several of the output parameter measurements are assumed to be for two-port
networks. When the network has 3 or more ports, the measurements are still
carried out by assuming that port=1 is the input and port=2 is the output. All
other ports are assumed terminated in their (noiseless) characteristic (z0)
impedances. Note that this assumption is equivalent to operating on the twoport [S] sub-matrix extracted from the multi-port [S] matrix. This is true for both
signal and noise calculations. A warning message is issued in cases where
N>2 when two-port quantities are requested.
Signal and noise port-wise calculations do not require that port elements use a
ground reference. Measurements are therefore possible; for example, for fully
differential circuits.
Since Zopt and Yopt can commonly take on infinite values when computing
optimum noise conditions, calculations for optimum noise loading is performed
in terms of the reflection coefficient GammaOpt, and is made as robust as
possible.
Output Format for Two-Port Noise Parameters in .sc* Files
The output of two-port noise parameter data in .sc* files are slightly modified.
The tabulated data appears with the following quantities in the following order:
*| 2-port noise parameters
*| frequency Fmin[dB] GammaOpt(M) GammaOpt(P)
*|
{...data...}
RN/Z0
Where
■
Fmin[dB] is the minimum noise figure (dB)
■
GammaOpt(M) is the magnitude of reflection coefficient needed to realize
Fmin
■
GammaOpt(P) is the phase (degrees) of reflection coefficient needed to
realize Fmin
■
RN/Z0 is the normalized noise resistance
Both GammaOpt and RN/Z0 values are normalized with respect to the
characteristic impedance of the port=1 element; for example, Z01.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
369
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
VSWR
The Voltage Standing Wave Ratio represents the ratio of maximum to minimum
voltages along a standing wave pattern due to a port’s impedance mismatch.
All ports other than the port of interest terminate in their characteristic
impedances. VSWR is a real number related to that port’s scattering
parameter:
1 + s ii
VSWR [ i ] = ----------------1 – s ii
ZIN(i)
The Input Impedance at the i port is the complex impedance into a port with all
other ports terminated in their appropriate characteristic impedance. It is
related to that port’s scattering parameter:
1 + S ii
ZIN [ i ] = Z 0i --------------1 – S ii
YIN(i)
The Input Admittance at the i port is the complex admittance into a port with all
other ports terminated in their appropriate characteristic impedance. It is
related to that port’s scattering parameter:
1 1 – S ii
YIN [ i ] = ------- --------------Z 0i 1 + S ii
K_STABILITY_FACTOR (Rollett Stability Factor)
The Rollett stability factor is:
2
2
2
1 – s 11 – s 22 + Δ
K = -------------------------------------------------------2 s 12 s 21
Δ determines the two-port S matrix calculated from this equation:
Δ = s 11 s 22 – s 12 s 21
An amplifier where K>1 is unconditionally stable at the selected frequency.
370
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
MU_STABILITY_FACTOR (Edwards-Sinsky Stability Factor)
The following equation defines the Edwards-Sinsky stability factor.
2
1 – |S 11 |
μ = ----------------------------------------------------* |+ |S 21S 12|
|S 22 – ΔS 11
Δ = S 11 S 22 – S 12 S 21
An amplifier with μ>1 is considered unconditionally stable at the specified
frequency.
Maximum Available Power Gain—G_MAX
This is the gain value that can be realized if the two-port is simultaneously
conjugate-matched at both input and output (with no additional feedback):
s 21
2
--------- ⎛ K – K – 1⎞
G max =
⎠
s 12 ⎝
K is the Rollett stability factor. Special cases of G_MAX are handled in the
following manner:
■
If |S12|=0 and (|S11|=1 or |S22|=1), G_MAX=|S21|2
■
If |S12|=0 and |S11|≠1 and |S22|≠1, G_MAX=G_TUMAX
■
If |S12|≠0 and K≤ 1, G_MAX=G_MSG
When values for K≤ 1, the Maximum Available Power Gain is undefined, and
HSPICE RF returns the Maximum Stable Gain.
Maximum Stable Gain - G_MSG
For a two-port that is conditionally stable (K<1), the following equation
calculates the maximum stable gain:
s 21
G MSG = --------s 12
HSPICE® Simulation and Analysis User Guide
Y-2006.03
371
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
To achieve this gain, resistively load the unstable two-port so that K=1, and
then simultaneously conjugately match the input and output ports. G_MSG is
therefore equivalent to G_MAX with K=1. In terms of admittance parameters:
y 21
G MSG = ---------y 12
MSG is equivalent to the Maximum Available Power Gain if K=1.
Maximum Unilateral Transducer Power Gain —G_TUMAX
This is the highest possible gain that a two-port with no feedback (that is,
S12=0) can achieve.
2
s 21
G tumax = -----------------------------------------------------2
2
( 1 – s 11 ) ( 1 – s 22 )
Unilateral Power Gain—GU
This is the highest gain that the active two-port can ever achieve by embedding
in a matching network that includes feedback. The frequency where the
unilateral gain becomes unity defines the boundary between an active and a
passive circuit. The frequency is usually referred to as fmax, the maximum
frequency of oscillation.
To realize this gain, HSPICE RF neutralizes the feedback of the two-port, and
simultaneously conjugate-matches both input and output:
2
s 21
------- – 1
s 12
G U = -----------------------------------------------s
s 21
⎧ 21 ⎫
2K ------ – 2Re ⎨ ------- ⎬
s
⎩ s 12 ⎭
12
372
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
Simultaneous Conjugate Match for G_MAX
A simultaneous conjugate match is required at the source and load to realize
the Gmax gain value. The source reflection coefficient at the input must be:
B 12
B1
C ∗1
Γ 1 = --------- ------------- – --------------- – 1
2
C1 2 C1
2C 1
2
2
B 1 = 1 – s 22 + s 11 – Δ
2
∗
C 1 = s 11 – Δ s22
Δ = s 11 s 22 – s 12 s 21
The load reflection coefficient (G_MAX_GAMMA_2) is:
B 22
B2
C 2∗
Γ 2 = --------- ------------- – --------------- – 1
2
C2 2 C2
2C 2
In the preceding equation:
2
2
B 2 = 1 – s 11 + s 22 – Δ
2
∗
C 2 = s 22 – Δ s11
Δ = s 11 s 22 – s 12 s 21
You can obtain useful solutions only when:
B1
------------>1
2C 1
B2
----------->1
2C 2
These equations also imply that K>1.
HSPICE RF derives calculations for the related impedances and admittances
from the preceding values.
For G_MAX_Z1:
1 + Γ1
Z 1 = Z 01 --------------1 – Γ1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
373
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
For G_MAX_Z2:
1 + Γ2
Z 2 = Z 02 --------------1 – Γ2
For G_MAX_Y1
1 1 – Γ1
Y 1 = -------- --------------Z 01 1 + Γ 1
For G_MAX_Y2
1 1 – Γ2
Y 2 = -------- --------------Z 02 1 + Γ 2
Equivalent Input Noise Voltage and Current—IN2, VN2, RHON
For each analysis frequency, HSPICE RF computes a noise-equivalent circuit
for a linear two-port. The noise analysis assumes that all ports terminate in
noise-less resistances. For circuits with more than two ports, ports identified as
3 and above terminate, and the analysis considers only ports 1 and 2. The
noise-equivalent circuit calculation results in an equivalent noise voltage and
current, and their correlation coefficient. These values are:
VN2 = |v n |
2
IN2 = |i n |
2
i n v*n
RHON = ρ n = ------------------------2
2
|i n | |v n |
Equivalent Noise Resistance and Conductance—RN, GN
These measurements are the equivalent resistance and conductance that
would generate the equivalent noise voltage and current values at a
temperature of T0 = 290k in a 1 Hz bandwidth (that is, Δf = 1Hz ).
2
|v n |
RN = R n = ----------------4kT 0 Δf
374
2
|i n |
GN = G n = ----------------4kT 0 Δf
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
Noise Correlation Impedance and Admittance—ZCOR, YCOR
These measurements represent the equivalent impedance and admittance that
you can insert at the input of the noise-equivalent circuit to account for the
correlation between the equivalent noise voltage and the current values.
2
ZCOR = ρ n
|v n |
i*n v n
---------- = ------------ = R cor + jX cor
2
2
|i n |
|i n |
YCOR = ρ n
i nv n *
|i n |
--------- = ------------ = G cor + jB cor
2
2
|v n |
|v n |
2
ZOPT, YOPT, GAMMA_OPT – Optimum Matching for Noise
The equivalent input noise sources and their correlation make it possible to
compute the impedance, admittance, and reflection coefficient values that, if
presented at the input of the noisy two-port, result in the best noise
performance. These values are:
Z opt =
R
2
------n – X cor – jX cor
Gn
1 =
Y opt = --------Z opt
Gn
2
------ – B cor – jB cor
Rn
Z opt – Z 01
GAMMA_OPT=Γ opt = ----------------------Z opt + Z 01
Noise Figure and Noise Figure Minimum—NF, NFMIN
If you set the input source impedance to ZOPT, the two-port operates with the
minimum Noise Figure. The definition of Noise Figure (F) is unusual, because it
involves the available gain of the two-port and not its transducer gain. You can
express it in the following form:
Na
F = 1 + --------------------G a kT 0 Δf
■
Ga is the available power gain.
■
Na is the available noise power at the output of the two-port (due solely to
the two-port’s noise and not to the input impedance).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
375
Chapter 11: Linear Network Parameter Analysis
RF Measurements From .LIN
■
k is Boltzmann’s constant.
■
T0 is the 290 Kelvin reference temperature.
The NMIN minimum noise figure value is computed as:
⎛
R
2 ⎞
NFMIN = F min = 1 + 2G n ⎜ R cor + ------n – Xcor ⎟
Gn
⎝
⎠
where NFMIN≥1. For input source impedance values other than ZOPT, the
Noise Figure varies as a function of the input source reflection coefficient,
according to:
2
R n |Γ S – Γ opt |
F = F min + --------------------------------2
2Z 01 |1+Γ opt |
The HSPICE RF Noise Figure measurement (NF) returns the noise figure value
if the input terminates in the port characteristic impedance (that is, Γs = 0 ). This
value is:
Gn
R n |Γ opt |
2
NF = F min + --------------------------------= F min + -------- |Z 01 – Z opt |
2
Z
01
2Z 01 |1+Γ opt |
Associated Gain—G_As
HSPICE RF also includes a measurement named Associated Gain, which
assumes that the Γ s inout impedance is matched for the minimum noise figure
(that is, Γ s = Γ opt ), while the output is matched for the maximum gain.
2
2
s 21 ( 1 – Γ Opt )
G AS = --------------------------------------------------------------2
2
1 – s 11 Γ Opt ( 1 – s′ 22 )
s 12 s 21 Γ Opt
′ = s + ---------------------------In the preceding equation: s 22
22 1 – s Γ 11 Opt
376
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
Extracting Mixed-Mode Scattering (S) Parameters
Extracting Mixed-Mode Scattering (S) Parameters
In HSPICE RF, the .LIN analysis includes a keyword for extracting mixedmode scattering (S) parameters.
Syntax
.LIN … [ mixedmode2port= dd|dc|ds|cd|cc|cs|sd|sc|ss ]
The following keywords in a .PRINT and .PROBE statements specifies the
elements in the mixed mode S parameter matrices:
S|Y|Z<xy>nm<(t)>
Argument
Description
x, y
One of the following:
■
D (differential)
C (common)
■
S (single-ended)
For example:
■
■
SCC=common mode S parameters
SDC or SCD=cross mode S parameters
If you omit x,y, then HSPICE uses the value set for the
mixedmode2port.
■
Scc
Common-mode S parameters
Scd and Sdc
Mode-conversion or cross-mode S parameters
m, n
port number
type
One of the following:
■
■
■
■
■
DB: magnitude in decibels
I: imaginary part
M: magnitude (default)
P: phase in degree
R: real part
HSPICE® Simulation and Analysis User Guide
Y-2006.03
377
Chapter 11: Linear Network Parameter Analysis
Extracting Mixed-Mode Scattering (S) Parameters
Defaults
Availability and default value for the mixedmode2port keyword depends on
the port configuration.
Example 1
p1=p2=single
Where,
■
Available: ss
■
Default: ss
Example 2
p1=p2=balanced
Where,
■
Available: dd,cd,dc,cc
■
Default: dd
Example 3
p1=balanced p2=single
Where,
■
Available: ds,cs
■
Default: ds
Example 4
p1=single p2=balanced
Where,
378
■
Available: sd,sc
■
Default: sd
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
Extracting Mixed-Mode Scattering (S) Parameters
Output File Formats
An sc# file format for the mixed mode:
■
The S element model has additional keywords, such as mixedmodei and
idatatype, if the netlist includes one or more balanced ports.
■
The mixedmode2port keyword prints in the header line.
■
The other S Element keywords also appear in the header lines.
Touchstone format for the mixed mode:
The following lines for data mapping are added to the head of the Touchstone
output file if the netlist includes one or more balanced ports.
!
!
!
!
S11=SDD11
S12=SDD12
S13=SDC11
S14=SDC12
Two-Port Parameter Measurement
Two-port parameter measurement function takes the first 2 ports, then reads
the corresponding parameter with the drive condition specified by the
mixedmode2port keyword.
Output Format and Description
File Type
Description
*.ac#
Output from both the .PROBE and .PRINT statements.
*.printac#
Output from the .PRINT statement. This is available in HSPICE RF
only.
*.sc#
The extracted S parameters/2-port noise parameters are written to
a *.sc# file by using the S-element format. If you want to simulate the S
element, you can reference the *.sc# file in your netlist.
* N=numOfPorts DATA=numOfFreq NOISE=[0|1] GROUPDELAY=[0|1]
* NumOfBlock=numOfSweepBlocks NumOfParam=numOfSweptParameters
* MIXEDMODE=[0|1] DATATYPE=mixedModeDataTypeString
.MODEL mname S
HSPICE® Simulation and Analysis User Guide
Y-2006.03
379
Chapter 11: Linear Network Parameter Analysis
Extracting Mixed-Mode Scattering (S) Parameters
+ N=numOfPorts FQMODEL=SFQMODEL TYPE=S Zo=*** *** ...
.MODEL SFQMODEL SP N=numberOfPorts SPACING=POI
INTERPOLATION=LINEAR MATRIX=NONSYMMETRIC
+ DATA= numberOfData
+ freq1
+ s11real s11imag s12real s12imag ... s1Nreal s1Nimag
...
+ sN1real sN1imag ... sNNreal sNNimag
...
...
+ freqNumberOfData
+ s11real s11imag s12real s12imag ...s1Nreal s1Nimag
...
+ sN1real sN1imag ... sNNreal sNNimag
*
*
*
*
2-port noise parameter
frequency
Fmin [dB]
GammaOpt(M)
GammaOpt(P)
0.10000E+09
0.
1.0000
0.
1.0281
...
RN/Zo
The 2-port noise section starts with “*” so that you can include this file in your
HSPICE or HSPICE RF input netlists.
Features Supported
.LIN analysis in HSPICE and HSPICE RF supports the following features:
■
Automatic calculation of bias-dependent S, Y, and Z parameters. No
additional sources required.
■
Automatic calculation of noise parameters.
■
Automatic calculation of group delay matrices.
In addition, HSPICE RF supports all existing HSPICE RF models. For noise
analysis, HSPICE and HSPICE RF view port 1 as the input and port 2 as the
output.
380
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
Extracting Mixed-Mode Scattering (S) Parameters
Prerequisites and Limitations
The following prerequisites and limitations apply to .LIN analysis in HSPICE
RF:
■
Requires one .LIN statement to specify calculation options.
■
Requires one .AC statement to specify frequency sweep and parameter
sweep.
■
Requires at least one P element, numbered from port 1 to N.
■
For noise analysis, HSPICE RF views port 1 as the input and port 2 as the
output.
Reported Statistics for the Performance Log (HSPICE RF Only)
■
■
Simulation time
•
DC op time
•
Total simulation time
Memory used
•
Total memory
Errors and Warnings
■
If the circuit contains fewer than two P Elements and noisecalc=1, then the
2-port noise calculation is skipped.
■
If the circuit contains fewer than two P Elements, does not let you cannot
use the .PRINT, .PROBE, or .MEAS command with any two-port noise or
gain parameters.
■
If the circuit contains more than two P Elements, all two-port parameters are
computed. By default, port=1 is the input and port=2 is the output. All
other ports terminate in their reference impedances.
Example
.OPTION POST=2
.AC DEC 1 20MEG 20G
.LIN noisecalc=1
Pout outs gnd port=2 RDC=50 RAC=50 DC=0 AC=1 0
Pin ins gnd port=1 RDC=50 RAC=50 DC=0.5 AC=0.5 0
xlna_2_ ins outs lna
HSPICE® Simulation and Analysis User Guide
Y-2006.03
381
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
.subckt lna in out
rhspr5 in _n481 50
rhspr6 _n523 out 100
vvdd _n523 gnd dc=1.8
qhspnpn3 out _n481 gnd gnd bjtm1 area=3
.ends lna
.global gnd
.END
.NET Parameter Analysis
HSPICE or HSPICE RF uses the AC analysis results to perform network
analysis. The .NET statement defines Z, Y, H, and S parameters to calculate.
The following list shows various combinations of the .NET statement for
network matrices that HSPICE or HSPICE RF calculates:
.NET Vout Isrc
.NET Iout Vsrc
.NET Iout Isrc
.NET Vout Vsrc
([M]T represents
V = [Z]
[I]
I = [Y]
[V]
T
= [H]
[I1 V2]T
[V1 I2]
[I1 V2]T = [S]
[V1 I2]T
the transpose of the M matrix).
Note:
The preceding list does not mean that you must use combination (1) to
calculate Z parameters. However, if you specify .NET Vout Isrc,
HSPICE or HSPICE RF initially evaluates the Z matrix parameters. It then
uses standard conversion equations to determine S parameters or any other
requested parameters.
Figure 57 shows the importance of variables in the .NET statement. Here,
Isrc and Vce are the DC biases, applied to the BJT.
382
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
Figure 58
Network Parameter Configurations
Z -parameter: .NET V(C) IB
I2
Y-parameter: .NET I(Vc) VBE
I2
C
I1
I1
IB
+
V1
-
+
V2
-
IC
VBE
H-parameter: .NET I(Vc) IB
I2
IB
+
V1
-
+
V2
-
VCE
S-parameter: .NET V(C) VBE
I2
C
I1
+
V1
-
C
I2
I1
+
V2
-
VCE
VBE
+
V1
-
+
V2
-
I2
Example
To calculate the H parameters, HSPICE or HSPICE RF uses the .NET
statement.
.NET I(VC) IB
VC denotes the voltage at the C node, which is the collector of the BJT. With
this statement, HSPICE or HSPICE RF uses the following equations to
calculate H parameters immediately after AC analysis:
V1 = H11 ⋅ I1 + H12 ⋅ V2
I2 = H21 ⋅ I1 + H22 ⋅ V2
To calculate Hybrid parameters (H11 and H21), the DC voltage source (VCE)
sets V2 to zero, and the DC current source (IB) sets I1 to zero. Setting I1 and
V2 to zero, precisely meets the conditions of the circuit under examination: the
input current source is open-circuited, and the output voltage source shorts to
ground.
384
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
A data file containing measured results can drive external DC biases applied to
a BJT. Not all DC currents and voltages (at input and output ports) might be
available. When you run a network analysis, examine the circuit and select
suitable input and output variables. This helps you to obtain correctlycalculated results. The following example demonstrates HSPICE network
analysis of a BJT or HSPICE RF.
Network Analysis Example: Bipolar Transistor
This example is based on demonstration netlist net_ana.sp, which is available
in directory $<installdir>/demo/hspice/bjt:
BJT network analysis
.option post nopage list
+ newtol reli=1e-5 absi=1e4 468e/b3*[j.5(li=list)]TJT*r[(+ n)lvdc absi=1e47
HSPICE® Simulation and Analysis User Guide
Y-2006.03
385
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
.NET Parameter Analysis
Xij(z), ZIN(z), ZOUT(z), YIN(z), YOUT(z)
Parameter
Description
X
In HSPICE or HSPICE RF, can be Z (impedance), Y (admittance), H
(hybrid), or S (scattering).
ij
i and j identify the matrix parameter to print in HSPICE or HSPICE RF.
Value can be 1 or 2. Use with the X value above (for example, Sij, Zij, Yij,
or Hij).
ZIN
Input impedance. For the one-port network, ZIN, Z11, and H11 are the
same. (HSPICE or HSPICE RF).
ZOUT
Output impedance. (HSPICE or HSPICE RF).
z
Output type (HSPICE or HSPICE RF):
■
■
■
■
■
■
R: real part.
I: imaginary part.
M: magnitude.
P: phase.
DB: decibel.
T: group time delay (HSPICE RF does not support group time delays
in AC analysis output).
YIN
Input admittance. For a one-port network, YIN is the same as Y11.
(HSPICE or HSPICE RF).
YOUT
Output admittance. (HSPICE or HSPICE RF).
If you omit z, output includes the magnitude of the output variable. The output
of AC Analysis includes voltages and currents.
Example
.PRINT AC Z11(R) Z12(R) Y21(I) Y22 S11 S11(DB) Z11(T)
.PRINT AC ZIN(R) ZIN(I) YOUT(M) YOUT(P) H11(M) H11(T)
.PLOT
AC S22(M) S22(P) S21(R) H21(P) H12(R) S22(T)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
387
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
Bandpass Netlist: Network Analysis Results
This example is based on demonstration netlist fbpnet.sp, which is available in
directory $<installdir>/demo/hspice/filters:
file fbpnet.sp network analysis
*
* scattering parameters computations.
* input and output impedance computations.
* computation of frequecy where zin cross 50 ohm.
* computation of phase of zin when zin cross 50 ohm.
*
.options dcstep=1 post
*band pass filter
c1 in 2 3.166pf
l1 2 3 203nh
c2 3 0 3.76pf
c3 3 4 1.75pf
c4 4 0 9.1pf
l2 4 0 36.81nh
c5 4 5 1.07pf
c6 5 0 3.13pf
l3 5 6 233.17nh
c7 6 7 5.92pf
c8 7 0 4.51pf
c9 7 8 1.568pf
c10 8 0 8.866pf
l4 8 0 35.71nh
c11 8 9 2.06pf
c12 9 0 4.3pf
l5 9 10 200.97nh
c13 10 out 2.97pf
rx out 0 1e14
vin in 0 ac 1
.ac lin 250 200meg 300meg
.net v(out) vin rout=50 rin=50
.probe ac s11(db) s11(p) s21(db) s21(p)
.probe ac zin(m) zin(p)
.meas ac cross50 when zin(m)=50 td=230meg
.meas ac phase50 find zin(p) when zin(m)=50 td=230meg
.end
388
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
Figure 59
S11 Magnitude and Phase Plots
BAND-PASS NETLIST: HSPICE NETWORK ANALYSIS RESULTS
04/14/2003 18:31:54
FBPL.AC0
S11[dB]
0
-10.0
-20.0
S11 [LIN]
-30.0
-40.0
FBPL.AC0
S11[PHASE]
179.141
100.0
0
-100.0
-175.88
200.0x
220.0x
240.0x
260.0x
280.0x
300.0x
HERTZ [LIN]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
389
Chapter 11: Linear Network Parameter Analysis
.NET Parameter Analysis
Figure 60
ZIN Magnitude and Phase Plots
BAND-PASS NETLIST: HSPICE NETWORK ANALYSIS RESULTS
04/14/2003 18:31:54
FBPL.AC0
ZIN[MAG
120.0
100.0
80.0
60.0
ZIN [LIN]
40.0
20.0
FBPL.AC0
ZIN[PHASE
90_0
50_0
0
-50_0
-90_0
200.0x
220.0x
240.0x
260.0x
280.0x
300.0x
HERTZ [LIN]
390
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 11: Linear Network Parameter Analysis
References
References
[1] Goyal, Ravender. “S-Parameter Output From SPICE Program”, MSN & CT,
February 1988, pp. 63 and 66.
[2] Robert J. Weber "Introduction to Microwave Circuits", IEEE Press.
[3] Behzad Razavi, "Design of Analog CMOS Integrated Circuits", McGraw Hill.
[4] Reinhold Ludwig, Pavel Bretchko, "RF Circuit Design Theory and
Applications".
[5] G.D. Vendelin, Design of Amplifiers and Oscillators by the S-Parameter
Method, John Wiley & Sons, 1982.
[6] R.S. Carson, High-Frequency Amplifiers, 2nd Edition, John Wiley & Sons,
1982.
[7] G. Gonzalez, Microwave Transistor Amplifiers: Analysis and Design, 2nd
Edition, Prentice-Hall, 1997.
[8] M.L. Edwards and J.H. Sinsky, "A single stability parameter for linear 2-port
networks," IEEE 1992 MTT-S Symposium Digest, pages 885-888.
[9] H. Rothe and W. Dahlke, "Theory of noisy fourpoles", Proc. IRE, volume 44,
pages 811-818, June 1956.
[10] David E. Bockeman, “Combined Differential and Common-Mode Scattering
Parameters: Theory and Simulation,” IEEE trans. on MTT Volume 43,
Number 7, Jul. 1995.
[11] “Understanding Mixed Mode S parameters,”
http://www.si-list.org/files/tech_files/Understandmm.pdf
[12] Robert J. Weber "Introduction to Microwave Circuits", IEEE Press.
[13] Behzad Razavi, "Design of Analog CMOS Integrated Circuits", McGraw Hill.
[14] Reinhold Ludwig, Pavel Bretchko, "RF Circuit Design Theory and
Applications."
HSPICE® Simulation and Analysis User Guide
Y-2006.03
391
Chapter 11: Linear Network Parameter Analysis
References
392
HSPICE® Simulation and Analysis User Guide
Y-2006.03
12
12
Using Verilog-A
Describes how to use Verilog-A in HSPICE simulations.
Note:
You can use Verilog-A in both HSPICE and HSPICE RF simulations;
therefore, in the context of this chapter, “HSPICE” refers to both HSPICE
and HSPICE RF unless noted otherwise.
Verilog-A is used to create and use analog behavioral descriptions that
encapsulate high-level behavioral and structural descriptions of systems and
components.
The language allows the behavior of each model, or module, to be described
mathematically in terms of its ports and parameters applied to an instance of
the module. A module can be defined at a level of abstraction appropriate for
the model and analysis, including architectural design, and verification. VerilogA supports both a top-down design as well as a bottom-up verification
methodology.
Verilog-A was derived from the IEEE 1364 Verilog Hardware Description
Language (HDL) specification and is intended for describing behavior in analog
systems. The Verilog-A language that HSPICE supports is compliant with
Verilog-AMS Language Reference Manual, Version 2.2, with limitations listed in
Unsupported Language Features on page 424.
The Verilog-A implementation in HSPICE supports a mixed design of Verilog-A
descriptions and transistor-level SPICE netlists with a simple use model. Most
analysis features available in HSPICE are supported for Verilog-A based
devices, including AC, DC, transient analysis, statistical analysis, and
optimization. The HSPICE RF supported analysis types are HB, HBOSC,
HBAC, HBNOISE, HBXF, PHASENOISE, and ENV.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
393
Chapter 12: Using Verilog-A
Getting Started
Getting Started
This section explains how to get started using a compact device model written
in Verilog-A in HSPICE.
Figure 61
HSPICE and Verilog-A
*Simple Verilog-A amplifier
.hdl amp.va
vs 1 0 1
rs 1 2 1
x1 2 3 va_amp gain=10
rl 3 0 1
module va_amp(in, out);
parameter real gain = 1.0;
electrical in, out;
analog begin
V(out) <+ gain * V(in);
end
endmodule
Verilog-A devices use the following conventions:
■
modules are loaded into the simulator with either the .HDL netlist command
or the –hdl command-line option (not supported in HSPICE RF).
■
modules are instantiated in the same manner as HSPICE subcircuits. The
first character for the name of instance should be “X”.
■
instance and model parameters can be modified in the same way as other
HSPICE instances.
■
module names should not conflict with any HSPICE built-in device keyword
(see Using Model Cards with Verilog-A Modules on page 410). If this
happens, HSPICE issues a warning message and ignores the Verilog-A
module definition.
■
node voltages and branch currents can be output using conventional output
commands.
To run an HSPICE Verilog-A simulation, you need to run the "hspice" script,
which is located in the $<installdir>/hspice_2006.03/bin/hspice, regardless of
the platform. For example,
/installed_hspice/hspice_2006.03/bin/hspice
The following example illustrates how a compact device model written in
Verilog-A can be analyzed with HSPICE.
Example: JFET Compact Device Model
HSPICE contains a large number of compact device models coded natively in
the simulator. Verilog-A provides a convenient method to introduce new
394
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Getting Started
compact models. The JFET device model uses a simple expression to relate
the source-drain current to the gate voltage.
The simplified Verilog-A description of this model is shown in below.
`include "constants.vams"
`include "disciplines.vams"
module jfet(d, g, s);
parameter real Vto = -2.0 from (-inf:inf); // Threshold voltage
parameter real Beta = 1.0e-4 from [0:inf);// Transconductance
parameter real Lambda = 0.0 from [0:inf); // Channel modulation
electrical d, g, s;
real Id, Vgs, Vds;
analog begin
Vgs = V(g,s);
Vds = V(d,s);
if (Vds <= Vgs-Vto)
Id = Beta*(1+Lambda*Vds)*Vds*(2*(Vgs-Vto)- Vds);
else if (Vgs-Vto < Vds)
Id = Beta*(1+Lambda*Vds)*(Vgs-Vto)*(Vgs-Vto);
I(d,s) <+ Id;
end
endmodule
In this example the module name is jfet and the module has three ports, named
d, g, and s. Three parameters, Vto, Beta, and Lambda, can be passed in from
the netlist. The electrical behavior is defined between the analog begin and end
statements. The node voltages across the gate to source and drain to source is
accessed and assigned to the variables Vgs and Vgd. These values are used
to determine the drain-source current, Id. The calculated current is contributed
to the branch from d to s in the final statement using the contribution operator,
<+.
This Verilog-A module is loaded into HSPICE with an .HDL command in the
netlist. The device is then instantiated using the X prefix for the device name.
The connectivity, module name, and parameter assignments follow the format
of a subcircuit device. The following instantiation line in the netlist is for this
device:
x1 drain gate source jfet Beta=1.1e-4 lambda=0.01
The nodes drain, gate, and source are mapped to the ports d, g, s in the same
order as defined in the module definition. Any parameters in the instantiation
line are passed to the module; otherwise, the default value defined on the
parameter declaration line is used. The parameter declaration allows ranges
and exclusions to be easily defined.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
395
Chapter 12: Using Verilog-A
Introduction to Verilog-A
@ ( initial_step ) begin
/*
Code inside an initial_step block is executed
at the first step of each analysis */
end
real_var = I(port1); // Current port1 to ground
V(bus[0], bus[1]) <+ real_var * real_param * int_param;
@ ( final_step ) begin
/* Code inside an final_step block is executed
at the last step of each analysis */
end
end
endmodule
Data Types
Four Verilog-A data types are available. The parameter type is used to pass
values from the netlist to the module.
Table 47
398
Verilog-A Data Types
Data Type
Description
attribute
A mechanism for specifying properties about objects, statements, and
groups of statements that may be used to control the operation or
behavior of the tool.
(* attr_spec {, attr_spec } *)
genvar
Special integer-valued variable for behavioral looping constructs
genvar genvar_name {, genvar_name};
integer
Discrete numerical type
integer integer_name {, integer_name};
local
parameters
Identified by the localparam keyword, local parameters are identical to
parameters except that they cannot directly be modified with the
defparam statement or by the ordered or named parameter value
assignment. Local parameters can be assigned to a constant
expression containing a parameter that can be modified with the
defparam statement or by the ordered or named parameter value
assignment.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Table 47
Verilog-A Data Types (Continued)
Data Type
Description
parameter
Attribute that indicates data type is determined at module instantiation.
parameter [{integer | real }] param_name =
default_value [ from[ range_begin:range_end ] [
exclude exclude_value_or_range ] ] ;
parameter
aliases
Aliases can be defined for parameters. This allows an alternate name
to be used when overriding module parameter values; for example,
parameter real dtemp = 0 from [-‘P_CELSIUS0:inf);
aliasparam trise = dtemp;
Then the following two instantiations of the module are valid:
nmos #(.trise(5)) m1(.d(d), .g(g), .s(s), .b(b));
nmos #(.dtemp(5)) m2(.d(d), .g(g), .s(s), .b(b));
And the value of the parameter dtemp, as used in the module equations
for both instances, is 5.
real
Continuous numerical type
real real_name {, real_name};
string
parameters
String parameters can be declared. Strings are useful for parameters
that act as flags, where the correspondence between numerical values
and the flag values may not be obvious. The set of allowed values for
the string can be specified as a comma-separated list of strings inside
curly braces.
Analog Operators and Filters
Analog operators and filters maintain memory states of past behavior. They can
not be used in an analog function.
Table 48
Verilog-A Analog Operators and Filters
Operator
Description
Time derivative
The ddt operator computes the time derivative of its argument.
ddt(expr)
Time integral
The idt operator computes the time-integral of its argument.
idt(expr, [ic [ , assert [ , abstol ] ] ] )
HSPICE® Simulation and Analysis User Guide
Y-2006.03
399
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Table 48
Verilog-A Analog Operators and Filters (Continued)
Operator
Description
Derivative
The ddx operator provides access to symbolically-computed
partial derivatives of expressions in the analog block.
ddx(expr, V(a)))
Linear time delay
absdelay() implements the absolute transport delay for
continuous waveform.
absdelay(input, time_delay [, maxdelay ])
Discrete
waveform filters
The transition filter smooths out piecewise linear waveforms.
transition(expr[,td[,rise_time[,fall_time
[,time_tol]]]])
The slew analog operator bounds the rate of change (slope) of
the waveform.
slew(expr[,max_pos_slew_rate
[,max_neg_slew_rate]])
The last_crossing() function returns a real value representing the
simulation time when a signal expression last crossed zero.
last_crossing(expr, direction)
Laplace
transform filters
laplace_zd() implements the zero-denominator form of the
Laplace transform filter. The laplace_np() implements the
numerator-pole form of the Laplace transform filter. laplace_nd()
implements the numerator- denominator form of the Laplace
transform filter. laplace_zp() implements the zero-pole form of the
Laplace transform filter.
laplace_*(expr, u, v)
Z-transform filters The Z-transform filters implement linear discrete-time filters. All Ztransform filters share three common arguments: T, t, and t0. T
specifies the period of the filter, is mandatory, and must be
positive. t specifies the transition time, is optional, and must be
nonnegative.
■
zi_zd() implements the zero-denominator form of the Ztransform filter.
■
zi_np() implements the numerator-pole form of the Ztransform filter.
■
zi_nd() implements the numerator-denominator form of the Ztransform filter.
■
zi_zp() implements the zero-pole form of the Z-transform filter.
zi_*( expr , u , v , T [ , t [ , t0 ] ] )
400
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Table 48
Verilog-A Analog Operators and Filters (Continued)
Operator
Description
Limited
Exponential
Limits exponential argument change from one iteration to the
next.
limexp(arg)
Mathematical Functions
The following mathematical functions are available when using HSPICE with
Verilog-A.
Table 49
Verilog-A Mathematical Functions
Function
Description
Domain
Return Value
ln()
natural log
x>0
real
log(x)
log base 10
x>0
real
exp(x)
exponential
x<80
real
sqrt(x)
square root
x>=0
real
min(x,y)
Minimum of x and y
all x, y
If either is real, returns real,
otherwise returns the type of x,y.
max(x,y)
Maximum of x and y
all x, y
If either is real, returns real,
otherwise returns the type of x,y.
abs(x)
absolute value
all x
same as x
pow(x,y)
x**y
if x>=0, all
y; if x<0,
int(y)
real
floor(x)
Floor
all x
real
ceil(x)
Ceiling
all x
real
HSPICE® Simulation and Analysis User Guide
Y-2006.03
401
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Transcendental Functions
The following mathematical functions are available when using HSPICE with
Verilog-A.
Table 50
402
Verilog-A Transcendental Function
Function
Description
Domain
sin(x)
sine
all x
cos(x)
cosine
all x
tan(x)
tangent
x != n (pi/2), n is odd
asin(x)
arc-sine
-1<= x <= 1
acos(x)
arc-cosine
-1<= x <= 1
atan(x)
arc-tangent
all x
atan2(x,y)
arc-tangent of x/y
all x, all y
hypot(x,y)
sqrt(x**2 + y**2)
all x, all y
sinh(x)
hyperbolic sine
x < 80
cosh(x)
hyperbolic cosine
x < 80
tanh(x)
hyperbolic tangent
all x
asinh(x)
arc-hyperbolic sine
all x
acosh(x)
arc-hyperbolic
cosine
x >= 1
atanh(x)
arch-hyperbolic
tangent
-1 <= x <= 1
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Introduction to Verilog-A
AC Analysis Stimuli
The AC stimulus function produces a sinusoidal stimulus for use during a smallsignal analysis:
ac_stim( [ analysis_name [ , mag [ , phase ]]])
Noise Functions
The noise functions contribute noise during small-signal analyses. The
functions have an optional name, which the simulator uses to tabularize the
contributions.
Table 51
Verilog-A Noise Functions
Function
Description
White Noise
Generates a frequency-independent noise of power pwr.
white_noise(pwr[,name])
Flicker Noise
Generates a frequency-dependent noise of power pwr at 1 Hz which
varies in proportion to the expression 1/fexp.
flicker_noise(pwr,exp[,name])
Noise Table
Defines noise via a piecewise-linear function of frequency. Vector is
frequency, power pairs in ascending frequencies.
Noise_table(vector[,name])
Analog Events
The following analog events are available when using HSPICE with Verilog-A.
Table 52
Verilog-A Analog Event-Controlled Statements
Function
Description
Initial Step
Event trigger at first step of an analysis.
@(initial_step[(list_of_analyses)])
Final Step
Event trigger at last step of an analysis.
@(final_step[(list_of_analyses)])
HSPICE® Simulation and Analysis User Guide
Y-2006.03
403
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Table 52
Verilog-A Analog Event-Controlled Statements (Continued)
Function
Description
Cross
Zero crossing threshold detection.
cross(expr[,dir[,time_tol[,expr_tol]]]);
Timer
Generates analog event at specific time.
timer(start_time[,period[,time_tol]]);
Above
Generates an event when a specified expression becomes greater than
or equal to zero.
above(expr[,time_tol[,expr_tol]]);
Timestep and Simulator Control
These functions provide a mechanism to alert the simulator to discontinuities or
to limit the time step.
Table 53
Verilog-A Discontinuity and Time Step Limit Functions
Function
Description
Bound time step
Controls the maximum time step the simulator takes during a
transient simulation.
$bound_step( expression );
Announce
discontinuity
Provides the simulator information about known discontinuities to
provide help for simulator convergence algorithms.
$discontinuity [ ( constant_expression ) ] ;
System Tasks and I/O Functions
System functions provide access to system-level tasks as well as access to
simulator information.
Table 54
404
Verilog-A System Tasks and I/O Functions
Function
Description
$param_given
Returns 1 if the parameter was overridden by a module instance
parameter value assignment and 0 otherwise.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Table 54
Verilog-A System Tasks and I/O Functions (Continued)
Function
Description
$table_model
Models behavior of a system by interpolating between data points
that are samples of that system’s behavior.
$strobe
$display
$write
Displays simulation data when the simulator has converged on a
solution for all nodes using a printf() style format.
$strobe(args);
$fopen
Opens a file for writing and assigns it to an associated channel.
multi-channel_desc = $fopen("file");
$fclose
Closes a file from a previously-opened channel(s).
$fclose(multi-channel_descriptor);
$fstrobe
$fdisplay
$fwrite
Writes simulation data to an opened channel(s) when the
simulator has converged. Follows format for $strobe.
$fstrobe(multi-channel_descriptor,
"information to be written");
$dist_functions
Probabilistic distribution functions
$debug
Provides the capability to display simulation data while the analog
simulator is solving the equations.
$random
Provides a mechanism for generating random numbers.
random_function ::=
$random [ ( seed [, type_string] ) ] ;
Simulator Environment Functions
The environment parameter functions return simulator environment information
to the module. Return circuit ambient temperature in Kelvin.
Table 55
Verilog-A Environment Parameter Functions
Function
Description
Circuit
temperature
Returns circuit ambient temperature in Kelvin.
$temperature
HSPICE® Simulation and Analysis User Guide
Y-2006.03
405
Chapter 12: Using Verilog-A
Introduction to Verilog-A
Table 55
Verilog-A Environment Parameter Functions (Continued)
Function
Description
Time
Returns absolute time in seconds.
$abstime
Thermal
voltage
$vt can optionally have Temperature (in Kelvin) as an input
argument and returns the thermal voltage (kT/q) at the given
temperature. $vt without the optional input temperature argument
returns the thermal voltage using $temperature.
$vt [ (Temperature) ]
Analysis flag
Returns true (1) if current analysis matches any one of the passed
arguments.
$analysis(str {, str } )
Simulation
parameter
Returns the value of the named specified simulation parameter.
gmin = $simparam("gmin", 1.0);
Module Hierarchy
Modules can instantiate other modules so that networks of modules can be
constructed. Structural statements are used inside the module block but cannot
be used inside the analog block.
module_name #({.param1(expr){, .param2(expr})}
instance_name ({node {, node});
Example
my_src #(.fstart(100), .ramp(z)) u1 (plus, minus);
Parameter Sets
Parameter sets (paramsets) bring the concept of model cards directly into
Verilog-A. Paramsets allow sharing of a set of parameters among several
modules. They may also be chained allowing a common parameter set to be
used.
Example
paramset nch my_nmos; // default paramset
parameter real l=1u from [0.25u:inf);
parameter real w=1u from [0.2u:inf);
406
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Simulation with Verilog-A Modules
.l=l; .w=w; .ad=w*0.5u; .as=w*0.5u;
.level=3; .kp=5e-5; .tox=3e-8; .u0=650; .nsub=1.3e17;
.vmax=0; .tpg=1; .nfs=0.8e12;
endparamset
Simulation with Verilog-A Modules
When simulating with Verilog-A in HSPICE, you need to have the following
basic input files:
■
HSPICE netlist/model card (Mandatory)
■
Verilog-A model file (for example, *.va or *.vams file) or Compiled Model
Library file (*.cml) (Mandatory)
■
HSPICE Verilog-A feature setup options (Optional, but mandatory under
certain conditions)
Basic output files:
■
HSPICE standard output files
■
The *.val file, Verilog-A log file, which contains Verilog-A specific message
from compiling and simulating phase. The contents of *.val file is also
echoed to the *.lis file.
■
Compiled Verilog-A code (.cml file) (when Verilog-A modules are compiled
manually).
Loading Verilog-A Devices
This section describes loading Verilog-A modules into HSPICE and specifying
cell names for Verilog-A definitions. A module must be loaded before it can be
instantiated.
Verilog modules are loaded into HSPICE in one of two ways:
■
by including an .HDL statement in an HSPICE netlist
■
by using the -hdl command-line option (not supported in HSPICE RF).
Files can be in the current directory or specified via an absolute or relative path.
The Verilog-A file is assumed to have a *.va extension when only a prefix is
provided. For example, .hdl “model” looks for a model.va file and not a file
named “model”.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
407
Chapter 12: Using Verilog-A
Loading Verilog-A Devices
Use the -vamodel command-line option to specify cell names for Verilog-A
definitions (not supported in HSPICE RF).
For a description of the .hdl statement, see the .HDL command in the
HSPICE Command Reference. For a description of the -hdl and -vamodel
command-line options, see “HSPICE Command Syntax” in the HSPICE
Command Reference.
Verilog-A File Search Path
During a simulation, HSPICE searches in the current directory for Verilog-A
files. You can also provide a search path via either the -hdlpath commandline option (not supported in HSPICE RF) or the HSP_HDL_PATH environment
variable to have HSPICE search other directories for the files. The -hdlpath
HSPICE command-line option is provided for HSPICE Verilog-A use only,
which defines the search path specifically for Verilog-A files.
For a description of the -hdlpath command-line option, see “HSPICE
Command Syntax” in the HSPICE Command Reference.
When a Verilog-A file cannot be found in the current working directory or the
directory defined by -hdlpath, or there is no -hdlpath defined, HSPICE
searches directory defined by HSP_HDL_PATH for the Verilog-A file.
The directory search order for Verilog-A files is:
1. Current working directory
2. Path defined by -hdlpath
3. Path defined by HSP_HDL_PATH
The path defined by either -hdlpath or HSP_HDL_PATH can consist a set of
directory names. The path separator must follow HSPICE conventions or
platform conventions (“;” on UNIX). Path entries that do not exist are ignored
and no error or warning messages are issued.
Example
This example assumes the c-shell is used.
setenv HSP_HDL_PATH
408
/lib_path/veriloga
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Verilog-A File Loading Considerations
Several restrictions and issues must be considered when loading Verilog-A
modules:
■
You can place an .HDL statement anywhere in the top-level circuit. All
Verilog-A modules are loaded into the system prior to any device
instantiation.
■
An .HDL statement is not allowed inside a .subckt or IF-ELSEIF-ELSE
block; otherwise, the simulation will exit with an error message.
■
When a module to be loaded has the same name as a previously-loaded
module, or the names differ in case only, the latter one is ignored and the
simulator issues a warning message.
■
If a Verilog-A module file is not found or the Compiled Model Library (CML)
file has an incompatible version, the simulation exits and an error message
is issued.
Instantiating Verilog-A Devices
Verilog-A devices are X elements. A Verilog-A device can have zero or more
nodes and can accept zero or more parameter assignments. Verilog-A devices
also support the concept of a model card. In either instance statements or
model card statements, invalid parameters that are not predefined in the
Verilog-A module file are ignored. HSPICE issues a warning message on those
invalid parameters.
Syntax
X<inst> <nodes> moduleName|ModelName param=value
Verilog-A module definitions are unique in each HSPICE simulation. A VerilogA module that matches the name, or differs only in case of a previously loaded
module is ignored. A Verilog-A module definition is ignored if its name conflicts
with HSPICE built-in models.
For any X element, the default search order to find the cell definition is:
1. HSPICE subcircuit definition
2. Verilog-A model card
3. Verilog-A module definition
HSPICE® Simulation and Analysis User Guide
Y-2006.03
409
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Example
Suppose you have the following HSPICE netlist fragment:
.hdl "mydiode"
X1 a b mydiode
.model mydiode D …
In this example, the simulation fails even though the Verilog-A module
mydiode is loaded. The reason is that the simulator finds the model card
mydiode first, which is an HSPICE built-in 'D' model—not the Verilog-A model
the X1 statement is trying to locate.
Using Model Cards with Verilog-A Modules
The HSPICE Verilog-A device supports the concept of model cards, with similar
usage to HSPICE standard built-in devices. The Verilog-A module name should
not conflict with the following built-in device keywords. In the event of a conflict,
HSPICE issues a warning message and ignores the module definition.
AMP, C, CORE, D, L, NJF, NMOS, NPN, OPT, PJF, PLOT, PMOS, PNP, R, U,
W, SP
The model card type should be the same as the Verilog-A module name. Every
Verilog-A module can have one or more associated model cards.
Unlike built-in device model cards and instances, you can specify any module
parameter in Verilog-A model cards, instance statements, or inherited
parameter values from module definitions. Instance parameters always
override model parameters.
If the model card includes parameters that are not predefined in its associated
module file, HSPICE issues a warning message, ignores the definition, and
continues with the simulation.
Syntax
.model mname type <pname1= > <pname2= > <pname3= > …
410
Argument
Description
mname
User defined model name reference. Elements must use this name to
refer to this model card.
type
Model type, it must be the same as Verilog-A module name.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Argument
Description
pname#
Parameter name. Every parameter must be predefined in its associated
Verilog-A module with default parameter value set. For legibility, use
either blanks or commas to separate each assignment. Use a plus sign
(+) to start a continuation line.
Example
For the following examples, assume the following Verilog-A module is used:
module va_amp(in, out);
electrical in, out;
input in;
output out;
parameter real gain=1.0;
parameter real fc=100e6;
...
analog begin
...
Its associated model cards can then be:
.model myamp va_amp gain=2 fc=200e6
.model myamp2 va_amp gain=10
The instantiations of Verilog-A module va_amp are:
x1
x2
x3
x4
x5
n1
n3
n5
n7
n9
n2 myamp
n4 myamp gain=3.0
n6 myamp gain=2.0 fc=150e6
n8 myamp2 fc=300e6
n10 va_amp
■
Instance x1 inherits model myamp parameters (that is, gain=2,
fc=200e6).
■
Instance x2 inherits “fc=200e6” from model myamp, but overrides “gain”
with the value 3.0.
■
Instance x3 overrides all model myamp parameters.
■
Instance x4 inherits parameter “gain=10” from model myamp2, and
overrides parameter “fc”, which is an implicit parameter in myamp2.
■
Instance x5 does not use a model card and directly instantiates the VerilogA module va_amp and inherits all module va_amp default parameters,
which are "gain=1" and "fc=100e6”.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
411
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Restrictions on Verilog-A Module Names
Verilog-A module name cannot conflict with certain HSPICE built-in device
keywords. If a conflict occurs, HSPICE issues a warning message and the
Verilog-A module definition is ignored.
The following built-in device keywords cannot be used as Verilog-A module
names: AMP, C, CORE, D, L, NJF, NMOS, NPN, OPT, PJF, PLOT, PMOS, PNP,
R, U, W, SP
Overriding Subcircuits with Verilog-A Modules
If both a subcircuit and a Verilog-A module have the same case-insensitive
name, by default, HSPICE uses the subcircuit definition. This behavior can be
changed by setting vamodel options, either at the command line or in
a .OPTION statement. The vamodel options are not supported in HSPICE RF.
The VAMODEL option works on cell-based definitions only. Instance-based
overriding is not supported.
Netlist Option
Syntax
.OPTION vamodel[=name]
This option is not supported in HSPICE RF. The name is the cell name that
uses a Verilog-A definition rather than the subcircuit when both exist. Each
vamodel option can take no more than one name. Multiple names need
multiple vamodel options.
If no name is provided for the vamodel option, HSPICE uses the Verilog-A
definition whenever it is available.
Example 1
.option vamodel=vco
This example instructs HSPICE to use Verilog-A definition for all instantiations
of cell vco.
Example 2
.option vamodel=vco vamodel=chargepump
This example instructs HSPICE to use Verilog-A definition for all instantiations
of cell vco and cell chargepump.
412
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Example 3
.option vamodel
This example instructs HSPICE to always use the Verilog-A definition whenever
it is available.
Command-line Option
Syntax
-vamodel <name> -vamodel <name2> …
This command-line option is not supported in HSPICE RF. The name is the cell
name that uses a Verilog-A definition rather than subcircuit when both are exist.
Each command-line -vamodel option can take no more than one name.
Repeat -vamodel if multiple Verilog-A modules are defined.
If no name after -vamodel is supplied, then in any case the Verilog-A
definition, whenever it is available, overrides the subcircuit.
The following examples show various ways to set the option and the resulting
HSPICE behavior.
Example 1
hspice pll.sp –vamodel vco
This example instructs HSPICE to use Verilog-A definition for all instantiations
of cell vco.
Example 2
hspice pll.sp –vamodel vco –vamodel chargepump
This example instructs HSPICE to use Verilog-A definition for all instantiations
of cell vco and cell chargepump.
Example 3
hspice pll.sp –vamodel
This example instructs HSPICE to always use a Verilog-A definition whenever it
is available.
Disabling .OPTION vamodel with .OPTION spmodel
These options are not supported in HSPICE RF. Use the .OPTION spmodel
netlist option to switch back to the HSPICE definition. For example, if you
override the HSPICE definition with the Verilog-A definition using .OPTION
HSPICE® Simulation and Analysis User Guide
Y-2006.03
413
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
vamodel, use .OPTION spmodel during .ALTER analysis to revert to the
HSPICE definition, which is the same as the VAMODEL option. The SPMODEL
option works on cell-based definitions only. Instance-based overriding is not
supported.
Syntax
.OPTION spmodel[=name]
The name is the cell name that will use spice definition. Each spmodel option
can take no more than one name; multiple names need multiple spmodel
options.
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 is set, the cell of vco uses the Verilog-A
definition whenever it is available.
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.
Using Vector Buses or "Ports"
The Verilog-A language supports the concept of buses (vector ports), whereas
HSPICE does not. If you instantiate a module that has a vector port, the
connections to individual bus signals in the HSPICE netlist must be specified.
The Verilog-A module internally expands the vector port and connects them to
the signals inside the Verilog-A module.
Example
Given a Verilog-A module with a vector port defined:
module d2a(in, out);
electrical [1:4] in;
electrical out;
analog ...
414
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Its instantiation in HSPICE could be:
x1 in1 in2 in3 in4 o1 d2a
In this case, the nodes in1 through in4 are mapped to ports in[1] -> in[4],
respectively. If the bus in Verilog-A module is specified as electrical [4:1], then
the signals would be connected as in1 -> in4 to in[4] -> in[1], respectively.
Using Integer Parameters
HSPICE netlist parameters are all of type real. When an integer Verilog-A
parameter is assigned a real value, it is coerced to an integer value.
Implicit Parameter M Support
Verilog-A supports the multiplicity factor. A Verilog-A device can have
parameter that is not device specific:
M
Multiplicity factor
If a loaded Verilog-A module has parameter with the name of either “M” or “m”,
then that module parameter cannot be set in the instance line. The “M” or “m”
parameter in the instance line always means the "Multiplicity factor" parameter
and the appropriate multiplicity factor is applied to the Verilog-A device during
the simulation. The implicit device parameter scaling factor S and the
temperature difference between the element and circuit, DTEMP, are not
supported.
Module and Parameter Name Case Sensitivity
Verilog-A is case-sensitive, whereas HSPICE is case-insensitive. This places
certain restrictions on use in terms of module and parameter names and output
control.
Module Names
When an attempt to load a second module into the system with a module name
that differs from a previously loaded module by case only, then the second
module is ignored and a warning message is issued.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
415
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Module Parameters
Parameters in the same module with names that only differ by case cannot be
redefined in either Verilog-A instance line or Verilog-A .MODEL cards. HSPICE
issues an error message and exits the simulaton.
Example
In this example a simple amplifier accepts two parameters, gain and Gain, as
input to the module.
module my_amp(in, out);
electrical in, out;
parameter real gain = 1.0;
parameter real Gain = 1.0;
analog V(out) <+ (Gain+gain)*V(in);
endmodule
If you instantiate this module as:
x1 n1 n2 my_amp Gain=1
HSPICE cannot uniquely define the Gain parameter, so a warning message is
issued and the definition of Gain is ignored. This module can be instantiated as
is, provided neither the Gain nor gain parameter is assigned in the netlist.
Output Simulation Data
Verilog-A devices support the same output capabilities as built-in devices. You
can access the following Verilog-A device quantities via any of these HSPICE
output statements: .PRINT, .PLOT, .PROBE, .GRAPH, .DOUT, and so forth.
416
■
Port current
■
Port voltage
■
Internal node voltage (HSPICE only)
■
Internal named branch current (HSPICE only)
■
Internal module variables (HSPICE only)
■
Module parameters (HSPICE only)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
V() and I() Access Functions
You can access port voltage and internal node voltage of Verilog-A devices via
the V() function. Port current and internal branch currents can be accessed via
the I() function.
The internal nodes of Verilog-A devices are accessible via the V() function
when the full hierarchical name is provided. The port current and named
branches (on the instance base only) can be accessible via the I() function.
Examples:
For the following examples, assume the Verilog-A module definition fragment
is:
module va_fnc(plus, minus);
inout plus, minus;
electrical plus, minus;
electrical int1, int2;
branch (int1, int2) br1;
//creates an internal branch br1 between internal
//nodes int1 and int2;
analog begin
…
And the Verilog-A module may be instantiated in the netlist as:
x1 1 2 va_fnc
To print the current on Verilog-A device port name plus for the instance x1:
.print I(x1.plus)
The plus is the port name defined in Verilog-A module, not the netlist node
name.
To print the Verilog-A module internal node named int1 for the instance x1:
.print V(x1.int1)
If the va_fnc module is hierarchical and has a child instance called c1 with an
internal node int1 then the node int1 can be output as
.print V(x1.c1.int1)
That is, the full HSPICE instance name is concatenated with the full internal
Verilog-A instance name to form the complete name.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
417
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
During compilation of Verilog-A modules, the compiler optimizes some internal
branches out of the system such that these branches are not available for
output. HSPICE Verilog-A provides a compilation environment variable,
HSP_VACOMP_OPTIONS, with –B option being set, all internal named branches
in Verilog-A modules become accessible. However, making all internal
branches accessible may have negative impact on simulation performance;
turn on the option only when necessary.
Refer to section “Setting Environment option for HSPICE Verilog-A Compiler”
for examples of setting HSP_VACOMP_OPTIONS.
After HSP_VACOMP_OPTIONS –B is set, you can probe branch current with
HSPICE output commands. In the previous Verilog-A module, there is an
internal branch name br1 declared. To probe the branch current
.print I(x1.br1)
Output Bus Signals
Verilog-A bus signals can be accessed with HSPICE output commands using
the Verilog-A naming and accessing conventions.
Example
Given an example Verilog-A module:
module my_bus(in, out);
electrical in;
electrical [1:4] out;
…
And instantiated in the netlist as
x1 1 2 3 4 5 my_bus
then the values of the vector port out can be output by explicitly listing each
position.
.print v(x1.out[1]), v(x1.out[2]), v(x1.out[3]), v(x1.out[4])
Bus elements can also be specified using wildcards, as described in the
section Using Wildcards in Verilog-A (HSPICE only) on page 420.
418
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Output Internal Module Variables (HSPICE only)
Verilog-A internal variables, by default, are hidden from output. However,
module variables with a description or units attribute, or both, are known as
output variables, and HSPICE provides access to their values; for example,
suppose a module for a MOS transistor with the following declaration at module
scope provides the output variable cgs:
(* desc="gate-source capacitance", units="F" *) real cgs;
The cgs module variable can be printed just like a normal parameter variable.
In addition, HSPICE Verilog-A provides a compilation environment variable
HSP_VACOMP_OPTION, with -G option being set, you can use HSPICE output
command to access internal module variables of Verilog-A instances.
Syntax
Instance:internal_variable
Example
.print xva_vco:freq
This example outputs internal variable frequency value of Verilog-A instance
xva_vco.
Output Module Parameters (HSPICE only)
You can use HSPICE output commands to output parameter values for VerilogA instances.
Syntax
Instance:parameter
Example
.print xva_1:gain
This example outputs the gain parameter value for the xva_1 Verilog-A
instance.
Case Sensitivity in Simulation Data Output
When Verilog-A information is output via the HSPICE output commands, the
case of the node names associated with the quantities to be output is ignored.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
419
Chapter 12: Using Verilog-A
Instantiating Verilog-A Devices
Contributions from the Verilog-A noise sources that have the same name when
case is ignored are combined.
Example
I(d,s) <+ white_noise(4*k*T/R1, "thermalnoise");
I(d2,s2) <+ white_noise(4*k*T/R2, "ThermalNoise");
The two noise contributions are combined into one contribution called
thermalnoise in the output files.
Using Wildcards in Verilog-A (HSPICE only)
Verilog-A names support the use of wildcards to simplify using the output
commands.
Examples:
Given the Verilog-A module,
module test(p,n);
electrical p,n;
electrical int1, int2;
…
instantiated as
x1 1 2 test
then all of the internal nodes (in this case int1 and int2) can be printed using
the command:
.print v(x1.*)
All indices of a bus in the module:
module my_bus(in, out);
electrical in;
electrical [1:4] out;
…
Can be specified as:
x1 1 2 3 4 5 my_bus
.print v(x1.out[*])
.print v(x1.*)
420
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Using the Stand-alone Compiler
Both of the internal nodes, int1 and int2 for the child ch1 in the instance
x_par1 can be specified using
.print v(x_par1.ch1.int*)
The HSPICE .OPTION POST command does not output internal nodes from
Verilog-A modules. Use the wildcard feature to specify a Verilog-A instance if
you need to output all internal nodes.
Port Probing and Branch Current Reporting Conventions
When printing and reporting currents for Verilog-A devices, HSPICE follows the
same conventions when specifying the direction of current flow as in built-in
devices. A positive branch current implies that current is flowing into the device
terminal or internal branch.
Unsupported Output Function Features
The following output functions are not supported in this release:
■
Port probing: In( ), where n is the node number). Instead, you can use
I(instance.port_name_in_module).
■
Iall(): Instead, you can output all the terminal currents using a wild card.
■
Isub(): This is not applicable to Verilog-A components.
■
P() and Power(): Instead, you can use the $strobe Verilog-A function .
■
Nodal capacitance
■
Group delay
Using the Stand-alone Compiler
Verilog-A modules used in HSPICE simulations are automatically compiled and
cached by the simulator. You can compile files manually if you wish (to check
syntax for example). The Verilog-A compiler takes a Verilog-A file as an input
and produces a Compiled Model Library (CML) file, which is a platform-specific
shared library.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
421
Chapter 12: Using Verilog-A
Setting Environment Option for HSPICE Verilog-A Compiler
Example 1
hsp-vacomp resistor.va
The Verilog-A compiler, hsp-vacomp, compiles the Verilog-A module file
resistor.va, and produces a CML file resistor.cml in the same directory.
You can include the CML file in the same manner as the Verilog-A file in an
HSPICE netlist.
Example 2
.hdl "resistor.cml"
Note:
When a CML file is specified in the load command the compiler is never
invoked, even if the source file is modified.
Setting Environment Option for HSPICE Verilog-A Compiler
While Verilog-A modules are automatically compiled in HSPICE simulation, you
can set environment variable HSP_VACOMP_OPTIONS to control compiler
options from default setting.
Example 1
setenv HSP_VACOMP_OPTIONS –G
When –G is set, all internal variables are accessible for output.
Example 2
setenv HSP_VACOMP_OPTIONS –B
When –B is set, all internal named branches are accessible for output.
The Compiled Model Library Cache
The HSPICE Verilog-A solution provides the performance of a compiled
solution without the need for user intervention. The first time a Verilog-A source
file is loaded, or after a Verilog-A source file is modified, the system
automatically invokes the compiler. The Compiled Model Library (CML) is
automatically cached and subsequent simulations use this cached file and
bypass the compilation process. Although for the most part you do not need to
be concerned with the cache mechanism, you can control some aspects. You
can change the cache location, prevent caching, or delete the cache.
422
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
The Compiled Model Library Cache
Cache Location
By default the cache directory is located in your $HOME directory under the
hidden directory .hsp-model-cache
This directory holds a directory structure that indicates compiler version,
platform, and model directory.
Example
Given the load command
.hdl "/users/finn/modules/amp.va"
the compiler generates a CML file in
/users/finn/.hsp-modelcache/1.30/users/finn/modules/lib.<arch>/amp.cml
Where <arch> is one of hpux, sun, linux, and so on.
The location of the cache can be changed from the default value by setting the
environment variable HSP_CML_CACHE to an appropriate location.
Example
The following sets the environment variable HSP_CML_CACHE so that the
model cache is created under the my_local_cache directory.
setenv HSP_CML_CACHE /users/finn/my_local_cache
If the previous example were now simulated the CML file would be
/users/finn/my_local_cache/1.30/users/finn/modules/lib.<arch>
/amp.cml
Deleting the Cache
The cache structure is maintained unless you choose to delete it manually. You
can do this any time; HSPICE automatically recreates the cache when needed.
One reason to delete the cache is if a newer version of the HSPICE Verilog-A
compiler is used and the previous cache is no longer necessary. The cache can
be deleted using conventional operating system commands.
Example
To delete the default cache, from the operating system command prompt,
execute
rm –r ~/.hsp-model-cache
HSPICE® Simulation and Analysis User Guide
Y-2006.03
423
Chapter 12: Using Verilog-A
Unsupported Language Features
Unsupported Language Features
The following Verilog-A LRM 2.1 Language Features are not supported.
■
Escaped identifiers
real \bus+index; // Not supported
■
Derived natures described in LRM 2.1 section 3.4.1.1
For example, the following deriving the nature New_curr from Ttl_curr is not
supported.
nature Ttl_curr
units = "A" ;
access = I ;
abstol = 1u ;
endnature
// The derived nature is not supported:
nature New_curr : Ttl_curr
abstol = 1m ;
maxval = 12.3 ;
endnature
■
Input, output, and inout enforcement described in LRM 2.1, section 7.1.
module test(in,out);
electrical in,out;
input in;
output out;
real out_value;
analog begin
out_value = 1.0;
V(in) <+ out_value;
// Input node used as output
// is not prevented, V(in) will be
// assigned to out_value
end
endmodule
■
The defparam statement as described in LRM 2.1, section 7.2.1
For example:
module rc(n1, n2);
electrical n1, n2;
my_res r1 (n1, n2);
my_cap c1 (n1, n2);
endmodule
module my_res(n1, n2);
electrical n1, n2;
424
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Unsupported Language Features
parameter dev_temp = 27;
parameter res = 50;
parameter tcr = 1;
analog
V(n1,n2) <+ I(n1,n2)*res*tcr*($temperature-dev_temp);
endmodule
module my_cap(n1, n2);
electrical n1, n2;
parameter dev_temp = 25;
parameter cap = 1;
parameter tcc = 1;
analog
I(n1,n2) <+ cap*ddt(V(n1,n2))*tcc*($temperature
dev_temp);
endmodule
// defparam statement not supported
module annotate;
defparam
rc.r1.dev_temp = 30;
rc.c1.dev_temp = 25;
endmodule
■
Ordered parameter lists in hierarchical instantiation as described in LRM
2.1, section 7.2.2.
For example:
module module_a(out,out2);
electrical out,out2;
parameter real value1 = -10.0;
parameter real value2 = -20.0;
analog begin
V(out) <+ value1;
V(out2) <+ value2;
end
endmodule
module test_param_by_order(out,out2);
electrical out,out2;
parameter real value1 = -1.0;
parameter real value2 = -2.0;
// Ordered parameter lists are not supported:
module_a #(1,2) A1(out,out2);
// instead use:
module_a #(.value1(1),.value2(2)) A1(out,out2);
endmodule
HSPICE® Simulation and Analysis User Guide
Y-2006.03
425
Chapter 12: Using Verilog-A
Unsupported Language Features
■
Hierarchical and out-of-module-references as described in the LRM 2.1,
section 7.
In this example, the reference to example2.net inside the example1
module is not supported.
module example1;
electrical example2.net; // Feature not supported
endmodule
module example2;
electrical net;
endmodule
■
Vector ports, where the port expression defining the size of a port is a
parameter expression, as described in LRM 2.1 section 7.3.1.
In this example, the vector port range size must be a constant—not a
parameter value.
module test(out);
parameter integer size = 7 from [1:16];
electrical [0:size] out; // Feature not supported
analog begin
V(out[0]) <+ 0.0;
end
endmodule
■
The ‘timescale directive, as described in LRM 2.2, section 3.2.3.
`timescale 1ns/10ps
■
// Feature not supported
The $monitor function, as described in LRM 2.1, section 10.6.
$monitor("\nEvent occurred."); // Feature not supported
■
Parameters used to specify ranges for the generate statement, as
described in LRM 2.1, section C.19.3.
generate indexr_identifier (start_expr,end_expr[,incr_expr ])
■
Time tolerances on timer() and transition() functions, as described in LRM
2.1, section 6.5.7.3 and 4.4.9.1, respectively.
timer (start_time [, period [, time_tol ] ] ) ;
transition(expr[,td [,rise_time [,fall_time [,time_tol ] ] ] ])
■
426
The `default_discipline directive, as described in LRM 2.1, section
11.1.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Unsupported Language Features
In the following example, the ports in and out must have their discipline
explicitly declared.
`include "disciplines.vams"
`default_discipline electrical // Feature not supported
module test(in,out);
// in,out default to electrical
analog
V(out) <+ I(in);
endmodule
■
Access to HSPICE primitives from a Verilog-A module, as described in LRM
2.1, section E.2.
module spice_rc (p1,p2);
electrical p1, p2;
capacitor #(.c(3p)) C3 (p1, p2); // Feature not
// supported
resistor #(.r(1k)) R1 (p1, p2); // Feature not
// supported
endmodule
■
"random type-string" feature (10.2 - 10.3).
■
reg-strings as described in Section 2.6 of LRM.
■
String parameters are supported only from other Verilog-A modules, but not
from the HSPICE netlist level.
■
$mfactor, $xposition, $yposition, $angle, $hflip, $vflip
functions.
■
“paramset” instantiation from HSPICE netlists is supported, but instantiation
from hierarchical Verilog-A modules is not supported.
■
Output variables and string parameters on paramsets.
■
$port_connected function.
■
$limit function.
■
The following are limitations in HSPICE RF Verilog-A only:
•
$strobe in DC analysis
•
$simparam simulation parameter
•
@(final_step)
•
0 port module
HSPICE® Simulation and Analysis User Guide
Y-2006.03
427
Chapter 12: Using Verilog-A
Known Limitations
•
Delays (absdelay()), event-controlled constructs, memory states
(variables that hold their value between timesteps), and explicit timedependent functions are not supported in RF analyses.
Known Limitations
This section describes the known limitiations when using Verilog-A with
HSPICE.
analysis() Function Behavior
The analysis() function definition assumes that the operating point (OP)
analysis associated with any user-specified analysis is unique to that userspecified analysis.
For example, when you specify the following function, it must return 1 for AC
analysis and 1 for its underlying operation point (OP) analysis.
analysis("ac")
Similarly, analysis("tran") must return 1 for transient analysis and 1 for its
underlying OP analysis.
In HSPICE, a single "common" OP analysis is performed in the setup that is
outside the context of AC, transient, or other analyses. Since that OP is outside
the context of the user-specified analysis, the analysis() function does not know
the parent analysis type (during the OP analysis). The analysis("ac"),
analysis("tran"), and so on, returns 0 during this “common” OP analysis. You
can ensure that the analysis function returns true (1) during these analyses by
adding “static” to the list of functions.
Example
if ( analysis("ac") )
begin
// do something
end
428
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 12: Using Verilog-A
Known Limitations
Should be written as:
if( analysis("ac", "static") )
begin
// do something
end
The same is true for the “tran” and “noise” analysis names.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
429
Chapter 12: Using Verilog-A
Known Limitations
430
HSPICE® Simulation and Analysis User Guide
Y-2006.03
13
13
Simulating Variability
Introduces variability, describes how it can be defined in HSPICE, and
introduces the variation block.
Introduction
As semiconductor technologies migrate to ever smaller geometries and they
exhibit larger variations in device characteristics, it becomes more important to
simulate (or predict) the effects of these variations on circuit response.
Variations in device characteristics are expressed through variations on
parameter values of the underlying device models.
■
Monte Carlo analysis is typically used to find the variation in circuit response
as a result of the parameter variations.
■
DC mismatch analysis is an efficient method for simulating the effects of
local variations on the DC response.
To get satisfactory answers from these analyses, the target technology must
have been characterized for variability and the characterization data properly
converted to variation definitions on device model parameters.
How To Define Variability in HSPICE
Three approaches are available to define variability in HSPICE:
■
Defining variations on parameters; for example,
.param var=agauss(20,1.2,3)
For a discussion of this topic, see see Appendix A, Statistical Analysis.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
431
Chapter 13: Simulating Variability
Variation Blocks Replace Previous Approaches
■
Defining variations on models using lot and dev parameters in the model
file; for example,
vth0=0.6 lot/0.1 dev/0.02
For a discussion of this topic, see Appendix A, Statistical Analysis.
■
Defining a variation block; for example,
.variation
global and local variation definitions
.end_variation
For additional information, see Chapter 14, Variation Block.
Variation Blocks Replace Previous Approaches
The variation block approach is expected to replace the approaches of defining
variations on parameters and models, because it best fulfills the requirements
for simulating Nanometer technology devices.
The advantages of the variation block over previous solutions are:
432
■
The variation block consolidate variation definitions in single records
■
A clear distinction exists between global and local variations
■
Only global or only local variations can be selected
■
The syntax allows for defining a local variation as a function of device
geometry
■
A new type of Monte Carlo output file allows for data mining
■
Monte Carlo and DC mismatch analyses give consistent results.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
14
14
Variation Block
Describes the use model and structure of the variation block.
Overview
The characteristics of circuits produced in semiconductor processing are
subject to variability, as is the case for any other manufactured product. For a
given target technology, the nominal device characteristics are described with a
set of parameters, which applies to a certain device model (for example,
BSIM3). In HSPICE, the variability of the model parameters is described in a
so-called “variation block”. A variation block is a container for specifying
variations introduced by the effects in manufacturing on geometry and model
parameters.
For the purpose of dealing with variations in HSPICE, they are separated into
global variations, defined as variations from lot to lot, wafer to wafer and chip to
chip, and into local variations, which are defined for devices in proximity on the
same integrated circuit. Both classes can be described in the variation block in
a very flexible way by user-defined expressions. Since there are currently no
industry-wide standards for specifying process variability, this feature allows
each company to implement their own proprietary model for variability. The
variation block is generally provided by a modeling group, very similar to device
models (for example, BSIM), because it must be created specifically for each
technology from test circuits.
The structure of the variation block allows for building expressions to model
interdependence and hierarchy of the variations. For example, one random
variable can control the variation in oxide thickness of both PMOS and NMOS
devices, as it is generally the same for both types of devices.
Note that the earlier methods of specifying variation are not compatible with the
variation block. For controlling the behavior of variation blocks, see section on
options for controlling the behavior. The variation block is currently used for
HSPICE® Simulation and Analysis User Guide
Y-2006.03
433
Chapter 14: Variation Block
Variation Block Structure
Monte Carlo and DCmatch analyses; for a description of these analyses, see
Chapter 15, Monte Carlo Analysis and Chapter 16, DC Mismatch Analysis,
respectively.
For the functions available to build expressions as presented in the next
sections, see Built-In Functions and Variables on page 229.
Variation Block Structure
The structure of a variation block is:
.variation
Define options
Define common parameters that apply to all sub-blocks
.global_variation
Define the univariate independent random variables
Define additional random variables through
transformation
Define variations of model parameters
.end_global_variation
.local_variation
Define the univariate independent random variables
Define additional random variables through
transformation
Define variations of model parameters
.element_variation
Define variations of element parameters
.end_element_variation
.end_local_variation
.end_variation
This structure contains three parts:
■
general section
■
sub-block for global variations
■
sub-block for local variations
General Section
In the general section, options can be defined that control how the information
in the variation block is used. Also, parameters can be defined that apply to
434
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 14: Variation Block
Variation Block Structure
both sub-blocks; however, these cannot contain any distribution related
functions.
Control Options
At the beginning of the variation block, options can be specified, one per line.
■
Ignore_variation_block=yes
Previous methods of specifying variations on parameters and models are
not compatible with the variation block. By default, the contents of the
variation block are used and any other specification is ignored, thus no
changes are required in existing netlists other than adding the variation
block. If it is still desirable to run the previous style variations, then the option
ignore_variation_block can be used.
■
Ignore_local_variations=yes and
Ignore_global_variations=yes
For investigating the effects of global or local variations only.
■
Monte Carlo-specific options (see Chapter 15, Monte Carlo Analysis).
Some of these options are useful if a variation block is part of a model file that
you cannot edit. One option can be specified per line. For example,
option Ignore_local_variations=yes
Global and Local Variations Sub-Blocks
Within the global or local variations sub-blocks, univariate independent random
variables can be defined. These are random variables with specific distributions
over a certain sample space. Additional random variables can be generated
through transformations. These random variables form the basis for
correlations and complex distributions.
In both sub-blocks, variations on model parameters can be defined. This is
where global or local variations on the parameters of semiconductor devices
are specified.
A special section within the sub-block for local variations allows for defining
local variations on elements. This is either for specifying local temperature
variations or variations on generic elements that do not have a model, as used
early in the pre-layout design phase; for example, resistors and capacitors.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
435
Chapter 14: Variation Block
Variation Block Structure
Independent Random Variables
When describing variations, a basic normal (Gaussian) distribution is assumed,
unless otherwise specified explicitly. This default behavior is explained in later
sections. Other types of distributions or correlations must be modeled by using
independent random variables. These come from three basic distributions:
■
Uniform distribution: defined over the range from -0.5 to 0.5: U()
■
Normal distribution: with mean=0 and variance=1, default range +/-4: N()
■
User-defined cumulative distribution function: CDF(xyPairs)
If f(x) is the probability density of a random variable x, then the cumulative
distribution function is the integral of f(x). A cumulative distribution function
can be approximated by a piecewise linear function, which can be described
as a sequence of pairs of points [xi, yi]. The following rules apply:
a. at least two pairs are required
b.
white space or a comma is required between each number
c.
the CDF starts at zero: y1=0
d. CDF ends at one: yn=1
e. xi values must be monotonically increasing xi+1 > xi
f.
yi values must be monotonically non-decreasing yi+1 >= yi
g. the CDF must have zero mean: x1 = - xn
Example
parameter var=CDF(-0.1 0 -0.05 0.5 0.05 0.5 0.1 1.0)
436
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 14: Variation Block
Variation Block Structure
The distributions N() and U() do not accept any arguments.
The syntax for defining independent random variables is:
parameter
a=U()
b=N()
c=CDF(x1,y1,......xn,yn)
These distributions cannot be referenced within expressions; variables must be
assigned and the variables can be used within expressions.
Dependent Random Variables
To model distributions which are more complex than the ones which are
available through the predefined independent random variables,
transformations can be applied by using expressions on independent random
variables. A dependent variable can also be created as a function of more than
one independent random variable to express correlation.
Example 1
This example creates a random variable with normal distribution, with mean A
and standard deviation B.
parameter var=N()
Y='A + B * var '
Example 2
This example creates a random variable with a uniform distribution from D to E,
where D and E are arbitrary constants.
parameter var=U()
Y='0.5*(D+E) + (E-D) * var '
Example 3
This example creates a random variable with two peaks.
parameter a=N() b=N() c='a+2*sgn(b)'
HSPICE® Simulation and Analysis User Guide
Y-2006.03
437
Chapter 14: Variation Block
Variation Block Structure
Variations of Model Parameters
Variations on model parameters can be defined in both global and local subblocks. In the course of the simulation, these variations are then applied to the
specified device model parameters.
In the simplest case, a variation with normal distribution is described with the
following syntax:
model_type model_name model_parameter='Expression for
Sigma'
If the expression references only constants and parameters that evaluate to
constants, then a Gaussian variation with zero mean and a sigma equal to the
expression is automatically implied. A shorthand notation is used; for example,
parameter='expression'
The meaning of this is actually:
variation_in_parameter='expression'
For example, the following defines a normal distribution with sigma of 10 on the
parameter rsh of the resistor with model Rpoly.
.global_variation
R Rpoly rsh=10
.end_global_variation
In a more complex case, the variation is modeled as a dependency on one or
several previously defined random variables by using the following syntax:
model_type model_name model_parameter=
Perturb('Expression')
For example, the variable Toxvar in the following is used to model global
variations on oxide thickness and by definition has a normal distribution with
mean=0 and sigma=1. The pmos and the nmos models receive the same
random variable and apply the variation to the model parameter tox in different
amounts; the oxide thickness for the two models is correlated.
.global_variation
Parameter Toxvar =N()
Nmos nch tox=Perturb('7e-10*Toxvar')
Pmos pch tox=Perturb('8e-10*Toxvar')
.end_global_variation
These model types are currently supported: NMOS, PMOS, R, and C.
438
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 14: Variation Block
Variation Block Structure
Variations can only defined on parameters that are explicitly specified in the
device model, and are included in the following list:
Model
Parameters
BSIM3 (level 49) lint
wint
vth0
Vfb
tox
u0
nsub
BSIM4 (level 54) lint
wint
vth0
vfb
toxm
toxe
u0
R
dlr
dw
rsh
C
cox
del
capsw thick
nsub
For binned models, variations can be defined separately by specifying the
model name with the bin extension; for example, devices from bins 1 and 2
receive different variation on the parameter lint, which models length
variation:
nmos snps20N.1 lint=10n
nmos snps20N.2 lint=12n
Variations of Element Parameters
Devices are not only affected by variations in the underlying model parameters,
but also through variations of properties specified at instantiation of an
element, or variations on implied properties, such as local temperature. Also,
early in the design phase, passive devices sometimes have only a nominal
value, but no model yet, because no decision has been made on the particular
implementation. For these elements, variations can be specified on the implicit
value parameter; for example: R1 1 0 1k .
In the simplest case, when there are no dependencies or correlations, a
variation with normal distribution is described with the following syntax:
element_type element_parameter='Expression for Sigma'
If the expression references only constants and parameters that evaluate to
constants, then a Gaussian variation with zero mean and a sigma equal to the
expression is automatically implied. Note that a shorthand notation is used:
parameter='expression'
The meaning of this is actually:
variation_in_parameter='expression'
HSPICE® Simulation and Analysis User Guide
Y-2006.03
439
Chapter 14: Variation Block
Variation Block Structure
For example, the following defines a normal distribution with sigma of 10 on the
resistors without model:
.element_variation
R R=10
.end_element_variation
The currently supported element types and their parameters are:
Element Parameter
M
DTEMP2
R
Rval*1 DTEMP2
C
Cval*1 DTEMP2
Q
AREA DTEMP2
D
DTEMP2
L
Lval*1 DTEMP2
I
DCval
V
DCval
1. Asterisk "*" denotes implicit value
parameter.
2. The DTEMP parameter is implicit; it
does not have to be specified on the
element instantiation line.
Because different classes of devices might be affected differently, a selection
mechanism based on element name and model name is provided by using a
condition clause:
element_type(condition_clause) element_parameter=
'Expression for Sigma'
The condition clause allows for specifying variations on selected elements,
according to their name or associated model. Wildcard substitutions can be
indicated as “?” for single character and “*” for multiple characters. Examples
for condition clause syntax are:
element_type(model_name~='modelNameA')
element_type(element_name~='elNameB')
element_type(model_name~='modelNameC' OPERATOR element_name~='elNameD') par='exp'
element_type(model_name~='modelNameE' OPERATOR model_name~='modelNameF') par='exp'
element_type(element_name~='elNameG' OPERATOR element_name~='elNameH') par='exp'
440
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 14: Variation Block
Variation Block Structure
Where OPERATOR can be && (AND), || (OR). The operator “~=” stands for
“matches”.
All pattern matching operations are case-insensitive. A leading subcircuit prefix
is ignored when matching the element name.
Example
In this example, only resistor ra1 varies.
ra1 1 0 1k
rb1 2 0 1k
.variation
.local_variation
.element_variation
R(element_name~='ra*') R=20
.end_element_variation
.end_local_variation
.end_variation
In a more complex case, the variation is modeled as a dependency on one or
several previously defined random variables by using the following syntax:
element_type(condition_clause) element_parameter=
Perturb('Expression')
Example
In this example, only resistor ra2 is affected by the temperature variation
specified with a uniform distribution from 0 to 10 degrees (the resistor is located
next to a power device).
ra1 1 0 1k
rb1 2 0 1k
ra2 3 0 rpoly l=10u w=1u
rb2 4 0 rpoly l=10u w=1u
.model rpoly r rsh=100 tc1=0.01
.variation
.local_variation
.element_variation
parameter tempvar=U()
R(element_name~='ra*' && model_name~='rpoly')
+
dtemp=perturb('10*tempvar+5')
.end_element_variation
.end_local_variation
.end_variation
HSPICE® Simulation and Analysis User Guide
Y-2006.03
441
Chapter 14: Variation Block
Variation Block Structure
Absolute Versus Relative Variation
By default, the specified variation is absolute, which means additive to the
original model or element parameter; however, sometimes it is more
appropriate to specify relative variations that are defined by appending a space
and a “%” sign to the expression. The simulator divides the result of the
expression by 100, and multiplies by the original parameter value and the
random number from the appropriate generator to calculate the change.
Example
In this example, the variation on the threshold parameter vth0 is specified as
absolute (sigma of 80 or 70mV), the variation on the mobility u0 as relative (15
or 13 percent).
global_variation
nmos snps20N vth0=0.08 u0=15 %
pmos snps20P vth0=0.07 u0=13 %
.end_global_variation
Access Functions
Certain local variations depend on element geometry, as defined with
parameters at instantiation. The access function get_E allows for using these
parameters in expressions by using the following syntax:
get_E(element_parameter)
Where element_parameter is the name of an element parameter, which
must be defined on the instantiation line (except for the DTEMP parameter).
This access function is only supported for local variations, because it does not
make sense to define global variations as a function of an element value in the
context of semiconductor technology.
For example, the variation on the threshold is specified as inversely
proportional to the square root of the total area of the device, as calculated
from the product of the element parameters W, L, and M.
nmos nch vth0='1.234e-9/sqrt(get_E(W)*get_E(L)*get_E(M))'
Another function allows for accessing the values of global parameters by using
the following syntax:
get_P(global_parameter)
442
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 14: Variation Block
Variation Block Example
For example, the resistor variation is proportional to absolute temperature.
.temp 100
ra1 1 0 1k
.variation
.local_variation
.element_variation
R R='(273+get_P(temper))*0.25'
.end_element_variation
.end_local_variation
.end_variation
Variation Block Example
This variation block is used in the example netlists opampdcm.sp and
opampmc.sp.
Most pieces of this example are explained below:
Global variations on vth0 (absolute)
Global variations on u0 (relative)
Local variations on vth0 (absolute), as a function of device area
Local variations on u0 (relative), as a function of device area
Local variation on the implicit value of resistors (relative)
.variation
.global_variation
NMOS SNPS20N vth0=0.07 u0=10 %
PMOS SNPS20P vth0=0.08 u0=8 %
.end_global_variation
.local_variation
nmos snps20N vth0='1.234e-9/sqrt(get_E(W)*get_E(L)*get_E(M))'
+ u0='2.345e-6/sqrt(get_E(W)*get_E(L)*get_E(M))' %
pmos snps20P vth0='1.234e-9/sqrt(get_E(W)*get_E(L)*get_E(M))'
+ u0='2.345e-6/sqrt(get_E(W)*get_E(L)*get_E(M))' %
.element_variation
R r=10 %
.end_element_variation
.end_local_variation
.end_variation
HSPICE® Simulation and Analysis User Guide
Y-2006.03
443
Chapter 14: Variation Block
Variation Block Example
444
HSPICE® Simulation and Analysis User Guide
Y-2006.03
15
15
Monte Carlo Analysis
Describes Monte Carlo analysis in HSPICE.
Overview
Monte Carlo analysis is the generic tool for simulating the effects of variations
in device characteristics on circuit performance. The variations in device
characteristics are expressed as distributions on the underlying model
parameters. For each sample of the Monte Carlo analysis, random values are
assigned to these parameters and a complete simulation is executed,
producing one or more measurement results. The series of results from a
particular measurement represent a distribution, which can be characterized by
statistical terms; for example, mean value and standard deviation (σ ). With
increasing number of samples, the shape of the distribution gets better defined
with the effect that the two quantities converge to their final values.
A standard way of analyzing the results is by arranging them in bins. Each bin
represents how many results fall into a certain range (slice) of the overall
distribution. A plot of these bins is a histogram, which shows the shape of the
distribution as the number of results versus slice. As the number of samples
increases, the shape of the histogram gets smoother.
The ultimate interest of Monte Carlo simulation is to find out how the
distribution in circuit response relates to the specification. The aspect of yield is
considered here:
■
What is the percentage of devices which meet the specification?
■
Is the design centered with respect to the specification?
Closely related is the aspect of over-design. This is when the circuit
characteristics are within specification with a wide margin, which could be at
the expense of area or power and ultimately cost.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
445
Chapter 15: Monte Carlo Analysis
Overview
A typical design process is iterative, first for finding a solution which meets the
nominal specification, and then moving on to a solution that meets yield and
economic constraints, including the effects of variations in device
characteristics. In this optimization process, it helps to understand the
relationship of the design parameters to the circuit response, and the
relationships of the different types of circuit response. This information is
available after running Monte Carlo analysis and can best be presented by
Pairs Plots. This is a matrix of two-dimensional plots for investigating pair-wise
relationships and exploring the data interactively. HSPICE does not produce
such plots, but makes the necessary data available from Monte Carlo
simulation. Figure 63 shows an example of a Pairs Plot from a simple resistive
divider:
Figure 63
Pairs Plot example
Monte Carlo analysis is computationally expensive; therefore, other types of
analysis have been created that produce certain results more efficiently. For
cases where only the effects of local variations on the DC response of a circuit
is of interest, a method called DC mismatch (DCmatch) analysis can be used;
for a description of DCmatch, see Chapter 16, DC Mismatch Analysis.
446
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 15: Monte Carlo Analysis
Monte Carlo Analysis in HSPICE
Monte Carlo Analysis in HSPICE
Monte Carlo analysis has been available in HSPICE for some time and is
based on two approaches:
■
defining distributions on global parameters (using AGAUSS, GAUSS, UNIF,
and AUNIF) in a netlist; for example,
.param var=agauss(20,1.2,3)
■
defining distributions on model parameters using DEV and LOT constructs in
a model file; for example,
vth0=0.6 lot/0.1 dev/0.02
The above two methods are documented in Appendix A, Statistical Analysis.
To satisfy some key requirements for modern semiconductor technologies, a
new approach is available based on the variation block, which is described in
detail in chapter 14. This new approach is not compatible with the earlier ones;
see the section on options for ways to select one or the other method.
For the following discussion, refer to diagram in Figure 64. Sample number 1 of
a Monte Carlo analysis is always executed with nominal values and no
variation. For subsequent samples, HSPICE updates the parameters specified
for variation in the variation block with random values. For global variations, a
specified parameter is changed by the same random value for all elements that
share a common model. For local variation, the specified parameter is changed
by a different random value for each element. The changes due to global and
local variations are additive and are saved in a file for post-processing. When
all the elements have been updated, the simulation is executed and the
measurement results are saved. When all the requested samples have been
simulated, HSPICE calculates the statistics of the measurement results and
includes them in the run listing.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
447
Chapter 15: Monte Carlo Analysis
Monte Carlo Analysis in HSPICE
Figure 64
Monte Carlo analysis flow in HSPICE
Start
Index 1:
Simulate with nominal parameters
Global variation:
Add some random value to particular
parameter for all devices
Local variation:
Add different random value to
specified parameters for each device
Index n:
Simulate with variations applied
More
Done
Calculate statistics
End
Input Syntax
Monte Carlo analysis is always executed in conjunction with some other
analysis:
.DC MCcommand
.DC sweepVar start stop step sweep MCcommand
.AC type step start stop sweep MCcommand
.TRAN step stop MCcommand
448
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 15: Monte Carlo Analysis
Monte Carlo Analysis in HSPICE
Syntax for MCcommand:
MONTE =
+ <val |
+ list num |
+ val firstrun=num |
+ list(<num1:num2><num3><num4:num5>)>
Parameter
Description
val
Specifies the number of random samples to produce.
val
Specifies the sample number on which the simulation starts.
firstrun=num
list num
Specifies the sample number to execute.
list(<num1:
num2>
<num3>
<num4:
num5>)
Samples from num1 to num2, sample num3, and samples from num4
to num5 are executed (parentheses are optional).
The parameter values and results are always the same for a particular sample,
whether generated in one pass or using firstrun or the list syntax.
Therefore, Monte Carlo analyses can be split or distributed and the results
spliced together.
Examples
In these examples a DC sweep is applied to a parameter k. In the first case, 10
samples are produced. In the second case, five samples are produced, starting
with sample number 6. In the last two examples, samples 5, 6, 7 and 10 are
simulated.
.dc
.dc
.dc
.dc
k
k
k
k
start=2
start=2
start=2
start=2
stop=4
stop=4
stop=4
stop=4
step=0.5
step=0.5
step=0.5
step=0.5
HSPICE® Simulation and Analysis User Guide
Y-2006.03
monte=10
monte=5 firstrun=6
monte=list 5:7 10
monte=list(5:7 10)
449
Chapter 15: Monte Carlo Analysis
Simulation Output
Note that options for the previous Monte Carlo style are ignored when
simulations based on the variation block are executed.
Simulation Output
The output listing file contains a summary of the names of the models and
model parameters, as well as the elements and element parameters, that are
subject to global or local variations. For each sample, the measured results are
printed. Towards the end, the statistics for the measured data are shown.
Partial printout of an output listing:
MONTE CARLO DEFINITIONS
Global variations:
model
snps20n
snps20n
Local variations:
model
snps20n
snps20n
Element variations:
element
r1
parameter
vth0
u0
parameter
vth0
u0
parameter
r
*** monte carlo index =
1 ***
systoffset= 1.0857E-03
*** monte carlo index =
2 ***
systoffset= -2.6826E-04
.
.
MONTE CARLO STATISTICS
meas_variable = systoffset
mean =
1.0124m
varian = 504.8187n
sigma = 710.5059u
avgdev = 523.4913u
max
=
2.2942m
min
=-268.2590u
Measure commands cause simulation results to be saved for each sample,
along with its index number. Depending on the analysis type, the name of the
result file has an extension of ms#, ma#, or mt#, where the # denotes the
regular sequence number for HSPICE output files. In addition, the changes in
all parameter values subject to variation are saved in a file with an extension of
mcs#, mca#, or mct#, depending on the analysis type.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
451
Chapter 15: Monte Carlo Analysis
Simulation Output
The structure of this file is the same as for regular measure files. In the header
section, the names of the parameters are presented as follows:
■
for global variation on model parameter:
[email protected]_name(ID)
■
for local variation on model parameter:
[email protected][email protected]_name(ID)
■
for local variation on element parameter:
[email protected]_name(ID)
Where ID is a string for identifying the type of the parameter as follows:
First character
Second character
Third character
M
Model
G
Global
R
Relative
E
Element
L
Local
A
Absolute
Results for parameters that have absolute variation specified in the variation
block are reported as absolute deviation from the nominal value. Results for
parameters that have relative variation specified are reported as a relative
deviation in percent. The printed value for parameter “status” is “1” for a
successful simulation, and “0” for a failed simulation.
For example, a mcs# file:
index
1.0000
2.0000
[email protected]@MGA
[email protected]@MGR
[email protected]@[email protected] [email protected]@[email protected]
[email protected]@[email protected] [email protected]@[email protected]
[email protected]@ELR status alter#
0.
0.
0.
0.
0.
0.
0.
1.0
1.0000
4.299e-02
6.285e-02
2.113e-04
2.354e-04
-4.926e-05
4.965e-04
0.2185
1.0
1.0000
.
.
In this example, the changes due to the global variations on parameters vth0
(absolute) and u0 (relative) are reported first, then the changes on each device
due to local variations on the same parameters are reported next, and finally,
the local variation on the parameter r of the element r0 are reported. Note that
452
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 15: Monte Carlo Analysis
Application Considerations
the parameter value applied to the device for a particular sample is the nominal
value, plus the reported change due to global variations, plus the reported
change due to local variations.
The contents of this parameter file are useful for data mining. In connection
with the measured data in the regular output file, the relationship of circuit
response variation to parameter variation can be investigated by using, for
example, a Pairs plot as shown in Figure 63 on page 446.
If a simulation fails without creating a result, HSPICE currently substitutes the
results of the previous sample, which can be misleading when analyzing the
relationship between results and underlying parameters. The information in the
“status” column of the result file can be used to skip the incorrect data.
Application Considerations
If too large variations are applied, caused by the combinations of variation
specified in the variation block and the value of Normal_limit, some circuits
show abnormal behavior under these conditions and the simulation result can
be completely off or missing. This can distort the result statistics reported by
HSPICE at the end of the Monte Carlo simulation. Therefore, you should to
review the individual measurement results for outliers and analyze them
properly. For example, when plotting measurement results as a function of
index in CosmosScope, the outliers are readily apparent.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
453
Chapter 15: Monte Carlo Analysis
Application Considerations
454
HSPICE® Simulation and Analysis User Guide
Y-2006.03
16
DC Mismatch Analysis
16
Describes the use of DCmatch analysis.
Mismatch
Variations in materials and procedures are the source of differences in
characteristics of identically designed devices on the same integrated circuit.
These are random time-independent variations by nature and are collectively
called mismatch.
Mismatch is one of the limiting factors in analog signal processing. It affects
more and more circuit types as device dimensions and signal swings are
reduced. Mismatch is a function of the geometry of the devices involved, their
spatial relationship (distance and orientation) and their environment. Mismatch
does not include the effects of global variations, such as batch-to-batch or
wafer-to-wafer variations, nor the effects or device degradation. For cases
where the effects of local variation on DC response of a circuit are of interest, a
method called DC mismatch (DCmatch) analysis can be used.
DCmatch analysis is related to sensitivity and noise analyses, and requires
significantly less runtime than Monte Carlo analysis. Thus, DCmatch analysis
provides an efficient technique for the approximate computation of the effects
of variability on circuit DC solutions.
DCmatch Analysis
In DCmatch analysis, the combined effects of variations of all devices on a
specified node voltage or branch current are determined. The primary purpose
is to consider the effects of local variations (that is, for devices in close
proximity). DCmatch analysis also allows for identifying groups of matched
devices (that is, devices that should be implemented on the layout according to
HSPICE® Simulation and Analysis User Guide
Y-2006.03
455
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
special rules). A secondary result is calculated as the influence of global
variations, which is useful for investigating whether their effects on circuit
response are much smaller then the effects of local variations, when optimizing
a design.
DCmatch analysis is based on the following dependencies and assumptions:
■
variations in device characteristics are modeled through variations in the
underlying model parameters.
■
statistics of the model parameters exhibit Normal distributions.
■
no correlation exists between the variations of different parameters of a
single device, or between the same parameter for different devices.
■
effects on a circuit’s DC solution are small; therefore, these variations also
exhibit Normal distributions.
In HSPICE, the variations in model parameters are defined in the variation
block (see Chapter 14, Variation Block). Those definitions are used to calculate
the variation in DC response. DCmatch analysis runs either from a default
operating point or for each value of the independent variable in a single DC
sweep. The default output is in the form of tables containing the sorted
contributions of the relevant devices to the total variation, as well as information
on matched devices. In the current implementation, a heuristic algorithm makes
a best guess effort to identify matched devices. This means that the results are
suggestions only. In addition to the table, the total variation and contributions of
selected devices can be output using .PROBE and .MEASURE commands.
Input Syntax
.DCMATCH OUTVAR <THRESHOLD=T> <FILE=string>
+ <PERTURBATION=P> <INTERVAL=Int>
456
Parameter
Description
OUTVAR
Valid node voltages, the difference between node pairs, or branch
currents.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
Parameter
Description
THRESHOLD
Report devices with a relative variance 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.
■
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.
Note:
If more than one DCmatch analysis is specified per simulation, only the last
statement is used.
Example 1
In this example, 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.
.DCmatch V(9) V(4,2) I(VCC)
Example 2:
In this example, the variable XVal is being swept in the DC command, from 1k
to 9k in increments of 1k. DCmatch variations are calculated for the voltage on
node out. Tables with DCmatch results are generated for the set XVal={1K, 4K,
7K, 9K}.
.DC XVal Start=1K Stop=9K Step=1K
.DCmatch V(out) Interval=3
HSPICE® Simulation and Analysis User Guide
Y-2006.03
457
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
DCmatch Table Output
For each output variable and sweep point, HSPICE generates a result record,
that includes setup information, total variations, and a table with the sorted
contributions of the relevant devices. The individual entries are:
■
sweep or operating points for which the table is generated
■
name of the output variable
■
DC value of this output variable
■
values used for DCmatch options
■
output sigma due to combined global and local variations
σ
■
global
2
+σ
local
2
results for global variations
•
number of devices that had no global variability specified
•
output sigma due to global variations
•
table with parameter contributions
•
contribution sigma (volts or amperes)
•
contribution variance for ith parameter (in percent)
2
sigma ( i ) -------------------------------× 100
n
2
sigma
(
k
)
∑
1
•
cumulative variance through ith parameter (in percent)
i
∑1sigma ( k )
2
-------------------------------- × 100
n
2
sigma
(
k
)
∑
1
■
458
results for local variations
•
number of devices that had no local variability specified
•
output sigma due to local variations
•
number of devices that had local variance contributions below the
threshold value and were not included in the table
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
•
table with sorted device contributions
Contribution sigma (in volts or amperes). Values below 100nV or 1PA
are rounded to zero to avoid reporting numerical noise.
•
contribution variance for the ith device (in percent)
2
sigma ( i ) -------------------------------× 100
n
2
sigma
(
k
)
∑
1
The parameter “Threshold” applies to this column.
•
cumulative variance through ith device (in percent)
i
∑1sigma ( k )
2
-------------------------------- × 100
n
2
sigma
(
k
)
∑
1
The table also includes a suggestion on matched devices that should be
verified independently. Devices with the same number in the column “Matched
pair” are likely to be matched. Their layout should be reviewed for conformity to
established matching rules.
Example
sweep point = operating point
===============================================================
output = v(out) node voltage =
1.25V threshold = 1.000E-2
perturbation = 2.00
interval = 1
Output sigma due to global and local variations = 619.62uV
DCMATCH GLOBAL VARIATION
10 Devices had no Global Variability specified.
Output sigma due to global variations = 289.66uV
-------------------------------------------------------------Contribution
Contribution
Cumulative
Independent
Sigma(V)
Variance (%)
Variance (%)
Variable
227.94u
61.92
61.92
[email protected]
139.48u
23.19
85.11
[email protected]
109.93u
14.40
99.51
[email protected]
20.19u
485.62m
100.00
[email protected]
DCMATCH LOCAL VARIATION
10 Devices had no Local Variability specified
Output sigma due to local variations =
547.74uV
4 Devices with Contribution Variance larger than Threshold
--------------------------------------------------------------Contribution Contribution Cumulative
Matched
Device
Sigma(V)
Variance (%) Variance (%) pair
Name
HSPICE® Simulation and Analysis User Guide
Y-2006.03
459
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
295.88u
295.65u
252.09u
247.94u
6.49u
1.72u
658.15n
0.
29.18
29.13
21.18
20.49
14.03m
984.38u
144.37u
0.
29.18
58.31
79.50
99.98
100.00
100.00
100.00
100.00
1
1
2
2
0
0
0
0
xi82.mn1
xi82.mn2
xi82.mp4
xi82.mp3
xi82.mp5
xi82.mn7
xi82.mn6
xi82.mn8
Output From .PROBE and .MEASURE Commands
The different results produced by DCmatch analysis can be saved by using
.PROBE and .MEASURE commands, for the output variable specified on the
.DCMATCH command. If multiple output variables are specified, a result is
produced for the last one only. A DC sweep needs to be specified to produce
these kinds of outputs; a single point is enough.
The keywords available for saving specific results from DCmatch analysis are:
■
DCm_total
Output sigma due to global and local variations.
■
DCm_global
Output sigma due to global variations.
■
DCm_global(par)
Contribution of parameter “par” to output sigma due to global variations.
■
DCm_local
Output sigma due to local variations.
■
DCm_local(dev)
Contribution of device “dev” to output sigma due to local variations.
Syntax for .PROBE Command
A .PROBE statement in conjunction with .OPTION POST creates a data file
with waveforms that can be displayed in CosmosScope.
.PROBE
.PROBE
.PROBE
.PROBE
.PROBE
460
DC
DC
DC
DC
DC
DCm_total
DCm_global
DCm_local
DCm_global(ModelType,ModelName,ParameterName)
DCm_local(InstanceName)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
This type of output is useful for plotting the effects of mismatch as a function of
bias current, temperature, or a circuit parameter.
Examples
In the first example, the contribution of the variations on vth0 (threshold) of the
nmos devices with model SNPS20N is saved. In the second example, the
contribution of device mn1 in subcircuit X8 is saved.
.probe dcm_global(nmos,SNPS20N,vth0)
.probe dcm_local(X8.mn1)
Syntax for .MEASURE Command
With .MEASURE statements, HSPICE performs measurements on the
simulation results and saves them in a file with a .ms# extension.
.MEAS
.MEAS
.MEAS
.MEAS
.MEAS
.MEAS
.MEAS
DC
DC
DC
DC
DC
DC
DC
res1
res2
res3
res4
res5
res6
res7
max DCm_total
max DCm_global
max DCm_local
max DCm_global(ModelType,ModelName,ParameterName)
max DCm_local(InstanceName)
find DCm_local at=SweepValue
find DCm_local(InstanceName) at=SweepValue
Example
In this example, the result systoffset reports the systematic offset of the
amplifier; the result matchoffset reports the variation due to mismatch; and the
result maxoffset reports the maximum (3-sigma) offset of the amplifier.
.MEAS DC systoffset avg V(inp,inn)
.MEAS DC matchoffset avg DCm_local
.MEAS DC maxoffset param='abs(systoffset)+3.0*matchoffset'
Practical Considerations
This section discusses practical considerations when using DCmatch analysis.
DCmatch Variability as a Function of Device Geometry
Various parameter relationships for device variability have been used in the
industry. Two approaches are shown below with their expressions for HSPICE.
The basic construct to calculate mismatch as a function of device size is get_E
(for details, see Access Functions on page 442).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
461
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
Example 1
This example assumes a standard transistor size and scales the variation with
the number of devices in parallel. This covers the practice of interdigitating
matched devices of a characterized standard size:
pmos pch vth0 ='dmvp0/sqrt(E(M))'
u0=’dmup0/sqrt(E(M))’ %
Example 2
This example shows an approach that calculates the variation as a function of
device size. Two of the three terms implement the well known dependence on
the inverse of the square root of the device area:
pmos pch vth0 =
+ 'dmpvtwl/sqrt(get_E(W)*get_E(L)*get_E(M)) +
+ dmpvtwll/(get_E(L)*sqrt(get_E(W)*get_E(M)))'
+ u0 ='dmpu0wl/sqrt(get_E(W)*get_E(L)*get_E(M)) %
Note that the HSPICE approach with user-defined expressions for sigma allows
for much more flexibility than the relationships shown in the above two
examples. For example, the variations due to body effect can easily be
included.
Parameter Traceability
The parameters and expressions are derived from characterizing dedicated
test structures for a given semiconductor technology. To use this information
successfully, it must be understood how it relates to the results from the
DCmatch analysis.
In the simple example considered in this discussion, variability is modeled as
threshold dependence only in the DCmatch definition block, VTH0 =dmvp0. It
is assumed that this VTH0 change maps directly to a VGS change. In the
characterization of the test structures, the differences in VGS for a transistor
pair at a certain current are collected and then, for example, the (one) sigma of
a large number of pairs is calculated as 1mV. The value for dmvp0 has to be
defined as 1mV / sqrt (2) = 0.707mV, because two devices are involved. After
simulating such a pair under the same conditions as for the characterization,
HSPICE reports a contribution of 0.707mV from each device, and a total
variation of sqrt (0.7072 + 0.7072 ) mV = 1mV between the two devices. This is
the same value as the original sigma from the test structure. For this flow to
work properly, it is crucial to know that
462
■
transistor pairs were measured
■
characterization results represent one sigma
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 16: DC Mismatch Analysis
DCmatch Analysis
■
DCmatch parameter value was adjusted for a single transistor
■
simulation results represent one sigma.
Of course, other scenarios are possible—it is just important to connect these
pieces properly to achieve correct results.
Example
An example netlist for running DCmatch analysis using a classic 7-transistor
CMOS operational amplifier. This example is available in the HSPICE demo
directory as $<installdir>/demo/hspice/apps/opampdcm.sp
In this netlist, device sizes are set up as a function of a parameter k, which
allows for investigating the effects of the global and local variations as a
function of device size. The following lines relate to DCmatch analysis:
...
.param k=2
...
mn1 net031 inn net044 nmosbulk snps20N L='k*0.5u' W='k*3.5u' M=4
mn2 net18 inp net044 nmosbulk snps20N L='k*0.5u' W='k*3.5u' M=4
mp3 net031 net031 vdda pmosbulk snps20P L='k*0.5u' W='k*4.5u' M=4
mp4 net18 net031 vdda pmosbulk snps20P L='k*0.5u' W='k*4.5u' M=4
...
.variation
.global_variation
nmos snps20N vth0=0.07 u0=10 %
pmos snps20P vth0=0.08 u0=8 %
.end_global_variation
.local_variation
nmos snps20N vth0='1.234e-9/sqrt(get_E(W)*get_E(L)*get_E(M))'
+
u0='2.345e-6/sqrt(get_E(W)*get_E(L)*get_E(M))' %
pmos snps20P vth0='1.234e-9/sqrt(get_E(W)*get_E(L)*get_E(M))'
+
u0='2.345e-6/sqrt(get_E(W)*get_E(L)*get_E(M))' %
.element_variation
R r=10 %
.end_element_variation
.end_local_variation
.end_variation
...
.dcmatch v(out)
.dc k start=1 stop=4 step=0.5
...
.meas DC systoffset find V(in_pos,in_neg) at=2
HSPICE® Simulation and Analysis User Guide
Y-2006.03
463
Chapter 16: DC Mismatch Analysis
References
.meas DC dcmoffset find DCm_local at=2
.meas DC maxoffset param='abs(systoffset)+3.0*dcmoffset'
.meas DC dcm_mn2 find DCm_local(xi82.mn2) at=2
.meas DC gloffset find DCm_global at=2
.option post
...
The DCmatch analysis produces four types of output from this netlist:
■
table from operating point with k=2 in the output listing
■
table from DC sweep for k=1 to 4 in file opampdcm.dm0
■
waveform for output variation as a function of k in file opampdcm.sw0
■
in file opampdcm.sw0 for k=2:
•
values for systematic offset
•
output sigma due to local variation
•
3-sigma amplifier offset
•
contribution of device mn2 to output sigma due to local variation
•
output sigma due to global variation.
References
[1] M.Pelgrom, A.Duinmaijer, and A.Welbers, “Matching Properties of MOS
Transistors,” IEEE J. Solid-State Circuits, vol. 24, no. 5, pp. 1433-1439, May
1989
[2] P.R.Kinget, “Device Mismatch and Tradeoffs in the Design of Analog
Circuits,” IEEE J. Solid-State Circuits, vol. 40, no. 6, pp. 1212-1224, June
2005
464
HSPICE® Simulation and Analysis User Guide
Y-2006.03
17
17
Optimization
Describes optimization in HSPICE for optimizing electrical yield.
Overview
Optimization automatically generates model parameters and component
values from a set of electrical specifications or measured data. When you
define an optimization program and a circuit topology, HSPICE automatically
selects the design components and model parameters to meet your DC, AC,
and transient electrical specifications.
The circuit-result targets are part of the .MEASURE command structure and you
use a .MODEL statement to set up the optimization.
Note:
HSPICE uses post-processing output to compute the .MEASURE
statements. If you set INTERP=1 to reduce the post-processing output, the
measurement results might contain interpolation errors. See the HSPICE
Command Reference for more information about these options.
HSPICE employs an incremental optimization technique. This technique solves
the DC parameters first, then the AC parameters, and finally the transient
parameters. A set of optimizer measurement functions not only makes
transistor optimization easy, but significantly improves cell and circuit
optimization.
To perform optimization, create an input netlist file that specifies:
■
Minimum and maximum parameter and component limits.
■
Variable parameters and components.
■
An initial estimate of the selected parameter and component values.
■
Circuit performance goals or a model-versus-data error function.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
465
Chapter 17: Optimization
Overview
If you provide the input netlist file, optimization specifications, component limits,
and initial guess, then the optimizer reiterates the circuit simulation until it either
meets the target electrical specification, or finds an optimized solution.
For improved optimization, reduced simulation time, and increased likelihood of
a convergent solution, the initial estimate of component values should produce
a circuit whose specifications are near those of the original target. This reduces
the number of times the optimizer reselects component values and resimulates
the circuit.
Optimization Control
How much time an optimization requires before it completes depends on:
■
Number of iterations allowed.
■
Relative input tolerance.
■
Output tolerance.
■
Gradient tolerance.
The default values are satisfactory for most applications. Generally, 10 to 30
iterations are sufficient to obtain accurate optimizations.
Simulation Accuracy
For optimization, set the simulator with tighter convergence options than
normal. The following are suggested options:
For DC MOS model optimizations:
absmos=1e-8
relmos=1e-5
relv=1e-4
For DC JFET, BJT, and diode model optimizations:
absi=1e-10
reli=1e-5
relv=1e-4
For transient optimizations:
relv=1e-4
relvar=1e-2
466
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Curve Fit Optimization
Use optimization to curve-fit DC, AC, or transient data:
1. Use the .DATA statement to store the numeric data for curves in the data
file as in-line data.
2. Use the .PARAM xxx=OPTxxx statement to specify the variable circuit
components and the parameter values for the netlist.
The optimization analysis statements use the DATA keyword to call the inline data.
3. Use the .MEASURE statement to compare the simulation result to the values
in the data file
In this statement, use the ERR1 keyword to control the comparison.
If the calculated value is not within the error tolerances specified in the
optimization model, HSPICE selects a new set of component values. HSPICE
then simulates the circuit again and repeats this process until it obtains the
closest fit to the curve or until the set of error tolerances is satisfied.
Goal Optimization
Goal optimization differs from curve-fit optimization, because it usually
optimizes only a particular electrical specification, such as rise time or power
dissipation.
To specify goal optimizations, do the following:
1. Use the GOAL keyword.
2. In the .MEASURE statement, select a relational operator where GOAL is the
target electrical specification to measure.
For example, you can choose a relational operator in multiple-constraint
optimizations when the absolute accuracy of some criteria is less important
than for others.
Timing Analysis
To analyze circuit timing violation, HSPICE uses a binary search algorithm.
This algorithm generate a set of operational parameters, which produce a
failure in the required behavior of the circuit. When a circuit timing failure
HSPICE® Simulation and Analysis User Guide
Y-2006.03
467
Chapter 17: Optimization
Overview
occurs, you can identify a timing constraint, which can lead to a design
guideline. Typical types of timing constraint violations include:
■
Data setup time before a clock.
■
Data hold time after a clock.
■
Minimum pulse width required to allow a signal to propagate to the output.
■
Maximum toggle frequency of the component(s).
Bisection Optimization finds the value of an input variable (target value)
associated with a goal value for an output variable. To relate them, you can use
various types of input and output variables, such as voltage, current, delay
time, or gain, and a transfer function.
You can use the bisection feature in either a pass-fail mode or a bisection
mode. In each case, the process is largely the same.
Optimization Statements
Optimization requires several statements:
■
.MODEL modname OPT ...
■
.PARAM parameter=OPTxxx (init, min, max)
Use .PARAM statements to define initial, lower, and upper bounds.
■
A .DC, .AC, or .TRAN analysis statement, with:
MODEL=modname
OPTIMIZE=OPTxxx
RESULTS=measurename
Use the .PRINT, .PLOT, and .GRAPH output statements, with
the .DC, .AC, or .TRAN analysis statements.
468
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Only use an analysis statement with the OPTIMIZE keyword for
optimization. To generate output for the optimized circuit, specify another
analysis statement (.DC, .AC, or .TRAN), and the output statements.
■
.MEASURE measurename ... <GOAL=| < | > val>
Include a space on either side of the relational operator:
=
<
>
For a description of the types of .MEASURE statements that you can use in
optimization, see Chapter 7, Simulation Output
The proper specification order is:
a. Analysis statement with OPTIMIZE.
b.
.MEASURE statements specifying optimization goals or error functions.
c.
Ordinary analysis statement.
d. Output statements.
Optimizing Analysis (.DC, .TRAN, .AC)
The following syntax optimizes HSPICE simulation for a DC, AC, and Transient
analysis.
.DC <DATA=filename> SWEEP OPTIMIZE=OPTxxx
+ RESULTS=ierr1 ... ierrn MODEL=optmod
.AC <DATA=filename> SWEEP OPTIMIZE=OPTxxx
+ RESULTS=ierr1 ... ierrn MODEL=optmod
.TRAN <DATA=filename> SWEEP OPTIMIZE=OPTxxx
+ RESULTS=ierr1 ... ierrn MODEL=optmod
Argument
Description
DATA
Specifies an in-line file of parameter data to use in optimization.
MODEL
The optimization reference name, which you also specify in the .MODEL
optimization statement.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
469
Chapter 17: Optimization
Overview
Argument
Description
OPTIMIZE
Indicates that the analysis is for optimization. Specifies the parameter
reference name used in the .PARAM optimization statement. In
a .PARAM optimization statements, if OPTIMIZE selects the parameter
reference name, then the associated parameters vary during an
optimization analysis.
RESULTS
The measurement reference name. You also specify this name in
the .MEASURE optimization statement. RESULTS passes the analysis
data to the .MEASURE optimization statement.
Optimization Examples
This section contains examples of HSPICE optimizations (for HSPICE RF
optimization, see “Optimization” in the HSPICE RF Manual):
■
MOS Level 3 Model DC Optimization
■
MOS Level 13 Model DC Optimization
■
RC Network Optimization
■
Optimizing CMOS Tristate Buffer
■
BJT S Parameters Optimization
■
BJT Model DC Optimization
■
Optimizing GaAsFET Model DC
■
Optimizing MOS Op-amp
MOS Level 3 Model DC Optimization
This example shows an optimization of I-V data to a Level 3 MOS model. The
data consists of gate curves (ids versus vgs) and drain curves (ids versus vds).
This example optimizes the Level 3 parameters:
470
■
VTO
■
GAMMA
■
UO
■
VMAX
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
■
THETA
■
KAPPA
After optimization, HSPICE compares the model to the data for the gate, and
then to the drain curves. .OPTION POST generates AvanWaves files for
comparing the model to the data.
Input Netlist File for Level 3 Model DC Optimization You can find the
sample netlist for this example in the following directory:
$installdir/demo/hspice/devopt/ml3opt.sp
The HSPICE input netlist shows:
■
Using .OPTION to tighten tolerances, which increases the accuracy of the
simulation. Use this method for I-V optimization.
■
.MODEL optmod OPT itropt=30 limits the number of iterations to 30.
■
The circuit is one transistor. The VDS, VGS, and VBS parameter names,
match names used in the data statements.
■
.PARAM statements specify XL, XW, TOX, and RSH process variation
parameters, as constants. The device characterizes these measured
parameters.
■
The model references parameters. In GAMMA= GAMMA, the left side is a
Level 3 model parameter name; the right side is a .PARAM parameter name.
■
The long .PARAM statement specifies initial, min and max values for the
optimized parameters. Optimization initializes UO at 480, and maintains it
within the range 400 to 1000.
■
The first .DC statement indicates that:
•
Data is in the in-line .DATA all block, which contains merged gate and
drain curve data.
•
Parameters that you declared as OPT1 (in this example, all optimized
parameters) are optimized.
•
The COMP1 error function matches the name of a .MEASURE statement.
•
The OPTMOD model sets the iteration limit.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
471
Chapter 17: Optimization
Overview
■
The .MEASURE statement specifies least-squares relative error. HSPICE
divides the difference between data par(ids) and model i(m1) by the larger
of:
•
the absolute value of par(ids), or
•
minval=10e-6
If you use minval, low current data does not dominate the error.
■
Use the remaining .DC and .PRINT statements for print-back after
optimization. You can place them anywhere in the netlist input file, because
parsing the file correctly assigns them.
■
The .PARAM VDS=0 VGS=0 VBS=0 IDS=0 statements declare these data
column names as parameters.
The .DATA statements contain data for IDS versus VDS, VGS, and VBS.
Select data that matches the model parameters to optimize.
Example
To optimize GAMMA, use data with back bias (VBS= -2 in this case). To
optimize KAPPA, the saturation region must contain data. In this example, the
all data set contains:
■
Gate curves: vds=0.1 vbs=0,-2 vgs=1 to 5 in steps of 0.25.
■
Drain curves: vbs=0 vgs=2,3,4,5 vds=0.25 to 5 in steps of 0.25.
Figure 65 shows the results.
472
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 65
Level 3 MOSFET Optimization
$LEVEL 8 MOSFET OPTIMIZATION
APRIL 22, 2004 4:58:09
OPTLEVELS.90
IM
ANP [LIN]
381.270U
300.0U
IO
200.0U
100.0U
ANP [LIN]
0
1.0
1.50
2.0
2.5
3.0
YOS [LIN]
3.5
4.0
4.50
5.0
5.0M
OPTLEVELS.90
IM
4.0M
IO
3.0M
2.0M
1.0M
250.0N
1.0
2.0
3.0
4.0
5.0
YOS [LIN]
MOS Level 13 Model DC Optimization
This example shows I-V data optimization to a Level 13 MOS model. The data
consists of gate curves (ids versus vgs) and drain curves (ids versus vds). This
example demonstrates two-stage optimization.
1. HSPICE optimizes the vfb0, k1, muz, x2m, and u00 Level 13 parameters
to the gate data.
2. HSPICE optimizes the MUS, X3MS, and U1 Level 13 parameters, and the
ALPHA impact ionization parameter to the drain data.
After optimization, HSPICE compares the model to the data. The POST option
generates AvanWaves files to compare the model to the data. Figure 66 on
page 476 shows the results.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
473
Chapter 17: Optimization
Overview
DC Optimization Input Netlist File for Level 13 Model This example is
based on demonstration netlist ml13opt.sp, which is available in directory
$<installdir>/demo/hspice/mos:
$LEVEL 13 mosfet optimization
$..tighten the simulator convergence properties
.OPTION nomod post=2 newtol relmos=1e-5 absmos=1e-8
.MODEL optmod OPT itropt=30
*Circuit Input
vds 30 0 vds
vgs 20 0 vgs
vbs 40 0 vbs
m1 30 20 0 40 nch w=50u l=4u
$..
$..process skew parameters for this data
.PARAM xwn=-0.3u xln=-0.1u toxn=196.6 rshn=67
$..the model and initial guess
.MODEL nch NMOS LEVEL=13
+ acm=2 ldif=0 hdif=4u tlev=1 n=2 capop=4 meto=0.08u
+ xqc=0.4
$...parameters obtained from measurements
+ wd=0.15u ld=0.07u js=1.5e-04 jsw=1.8e-09
+ cj=1.7e-04 cjsw=3.8e-10
$...parameters not used for this data
+ k2=0 eta0=0 x2e=0 x3e=0 x2u1=0 x2ms=0 x2u0=0 x3u1=0
$...process skew parameters
+ toxm=toxn rsh=rshn
+ xw=xwn xl=xln
$...optimized parameters
+ vfb0=vfb0 k1=k1 x2m=x2m muz=muz u00=u00
+ mus=mus x3ms=x3ms u1=u1
$...impact ionization parameters
+ alpha=alpha vcr=15
.PARAM
+ vfb0 = opt1(-0.5, -2, 1)
+ k1 = opt1(0.6,0.3,1)
+ muz = opt1(600,300,1500)
+ x2m = opt1(0,-10,10)
+ u00 = opt1(0.1,0,0.5)
+ mus = opt2(700,300,1500)
+ x3ms = opt2(5,0,50)
+ u1 = opt2(0.1,0,1)
+ alpha = opt2(1,1e-3,10)
474
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
*Optimization Sweeps
.DC DATA=gate optimize=opt1 results=comp1 model=optmod
.MEAS DC comp1 ERR1 par(ids) i(m1) minval=1e-04 ignor=1e-05
.DC DATA=drain optimize=opt2 results=comp2 model=optmod
.MEAS DC comp2 ERR1 par(ids) i(m1) minval=1e-04 ignor=1e-05
*DC Data Sweeps
.DC DATA=gate
.DC DATA=drain
*Print Sweeps
.PRINT DC vds=par(vds) vgs=par(vgs) im=i(m1) id=par(ids)
.PRINT DC vds=par(vds) vgs=par(vgs) im=i(m1) id=par(ids)
*DC Sweep Data
$..data
.PARAM vds=0 vgs=0 vbs=0 ids=0
.DATA gate vds vgs vbs ids
1.000000e-01 1.000000e+00 0.000000e+00 1.655500e-05
1.000000e-01 5.000000e+00 -2.000000e+00 3.149500e-04
.ENDDATA
.DATA drain vds vgs vbs ids
2.500000e-01 2.000000e+00 0.000000e+00 2.809000e-04
5.000000e+00 5.000000e+00 0.000000e+00 4.861000e-03
.ENDDATA
.END
HSPICE® Simulation and Analysis User Guide
Y-2006.03
475
Chapter 17: Optimization
Overview
Figure 66
Level 13 MOSFET Optimization
ANPORT.SP MOS OPERATIONAL AMPLIFIER OPTIMIZATION
APRIL 22, 2003 5:21:26
MLLSOPT.SV0
IM
ANP [LIN]
300.0U
IO
200.0U
100.0U
0
1.0
1.50
2.0
2.5
3.0
YOS [LIN]
3.5
4.0
4.50
5.0
MLLSOPT.SV1
IM
ANP [LIN]
4.9787M
4.0M
IO
3.0M
2.0M
1.0M
250.0M
1.0
2.0
YOS [LIN]
3.0
4.0
5.0
RC Network Optimization
The following example optimizes the power dissipation and time constant for an
RC network. The circuit is a parallel resistor and capacitor. Design targets are:
■
1 s time constant.
■
50 mW rms power dissipation through the resistor.
The HSPICE strategy is:
476
■
RC1 .MEASURE calculates the RC time constant, where the GOAL of .3679
V corresponds to 1 s time constant e-rc.
■
RC2 .MEASURE calculates the rms power, where the GOAL is 50 mW.
■
OPTrc identifies RX and CX as optimization parameters, and sets their
starting, minimum, and maximum values.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Network optimization uses these HSPICE features:
■
Measure voltages and report times that are subject to a goal.
■
Measure device power dissipation subject to a goal.
■
Measure statements replace the tabular or plot output.
■
Parameters used as element values.
■
Parameter optimizing function.
■
Transient analysis with SWEEP optimizing.
Example
This example is based on demonstration netlist rcopt.sp, which is available in
directory $<installdir>/demo/hspice/ciropt:
*file: rcopt.sp optimize the power dissapation and time constant
* of an rc network
*
* optimize to the goals of 1sec time constant and 50mwatts rms
power.
* optrc identifies rx and cx as optimization parameters and sets
* their starting, minimum, and maximum values. measure statement
rc1
* calculates the rc time constant. ( .3679=e**-rc ) where the
goal is
* rc=1sec. measure statement rc2 calculates the rms power where the
* goal is 50 milliwatts.
*
* hspice features used:
*
- measure voltages and report times subject to goal
*
- measure device power dissapation subject to goal
*
- element value parameterization
*
- parameter optimization function
*
- transient with sweep optimize
*
.option post
.param rx=optrc(.5, 1e-2, 1e+2)
.param cx=optrc(.5, 1e-2, 1e+2)
.measure tran rc1 trig at=0 targ v(1) val=.3679 fall=1 goal=1sec
.measure tran rc2 rms p(r1) goal=50mwatts
.model opt1 opt
.tran .1 2$ initial values
.tran .1 2 sweep optimize=optrc results=rc1,rc2 model=opt1
.tran .1 2$ analysis using final optimized values
HSPICE® Simulation and Analysis User Guide
Y-2006.03
477
Chapter 17: Optimization
Overview
The optimizer initially uses the Steepest Descent method as the fastest
approach to the solution. It then uses the Gauss-Newton method to find the
solution. During this process, the Marquardt Scaling Parameter becomes very
small, but starts to increase again if the solution starts to deviate. If this
happens, the optimizer chooses between the two methods to work toward the
solution again.
If the optimizer does not attain the optimal solution, it prints both an error
message, and a large Marquardt Scaling Parameter value.
Number of Function Evaluations:
This is the number of analyses (for example, finite difference or central
difference) needed to find a minimum of the function.
Number of Iterations:
This is the number of iterations needed to find the optimized or actual solution.
Optimized Parameters OPTRC
.param rx= 7.4823
.param cx=133.9934m
$
$
HSPICE® Simulation and Analysis User Guide
Y-2006.03
55.6965
44.3035
5.7945m
5.1872m
479
Chapter 17: Optimization
Overview
Figure 67
Power Dissipation and Time Constant (VOLT) RCOPT.TR0=Before
Optimization, RCOPT.TR1=Optimized Result
*FILE: RCOPT.SP OPTIMIZE THE POWER DISSIPATION AND TIME CONSTANT
APRIL 22, 2004 5:38:12
998.587N
RCOPT.TR0
1
900.0N
RCOPT.TR1
1
800.0N
VOLT [LIN]
700.0N
600.0N
500.0N
400.0N
300.0N
200.0N
100.0N
929.90U
480
0
200.0M
400.0M
600.0M
TIME [LIN]
800.0M
1.0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 68
Power Dissipation and Time Constant (WATT) RCOPT.TR0=Before
Optimization, RCOPT.TR1=Optimized Result
*FILE: RCOPT.SP OPTIMIZE THE POWER DISSIPATION AND TIME CONTSTANT
APRIL 22, 2004 5:38:12
RCOPT.TR0
PIR1
1.80
RCOPT.TR1
PIR1
1.60
MATT [LIN]
1.40
1.20
1.0
800.0M
600.0M
400.0M
200.0M
0
0
200.0N
400.0N
600.0N
TIME [LIN]
800.0N
1.0
Optimizing CMOS Tristate Buffer
The example circuit is an inverting CMOS tristate buffer. The design targets
are:
■
Rising edge delay of 5 ns (input 50% voltage to output 50% voltage).
■
Falling edge delay of 5 ns (input 50% voltage to output 50% voltage).
■
RMS power dissipation should be as low as possible.
■
Output load consists of:
•
pad capacitance
•
leadframe inductance
•
50 pF capacitive load
The HSPICE strategy is:
■
Simultaneously optimize both the rising and falling delay buffer.
■
Set up the internal power supplies, and the tristate enable as global nodes.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
481
Chapter 17: Optimization
Overview
■
Optimize all device widths except:
•
Initial inverter (assumed to be standard size).
•
Tristate inverter and part of the tristate control (optimizing is not
sensitive to this path).
■
Perform an initial transient analysis for plotting purposes. Then optimize and
perform a final transient analysis for plotting.
■
To use a weighted RMS power measure, specify unrealistically-low power
goals. Then use MINVAL to attenuate the error.
Input Netlist File to Optimize a CMOS Tristate Buffer This example is
based on demonstration netlist trist_buf_opt.sp, which is available in directory
$<installdir>/demo/hspice/apps:
*Tri-State input/output Optimization
.OPTION nomod post
+ defl=1.2u relv=1e-3 absvar=.5 relvar=.01
*Circuit Input
.global lgnd lvcc enb
.macro buff data out
mp1 DATAN DATA LVCC LVCC p w=35u
mn1 DATAN DATA LGND LGND n w=17u
mp2 BUS DATAN LVCC LVCC p w=wp2
mn2 BUS DATAN LGND LGND n w=wn2
mp3 PEN PENN LVCC LVCC p w=wp3
mn3 PEN PENN LGND LGND n w=wn3
mp4 NEN NENN LVCC LVCC p w=wp4
mn4 NEN NENN LGND LGND n w=wn4
mp5 OUT PEN LVCC LVCC p w=wp5 l=1.8u
mn5 OUT NEN LGND LGND n w= wn5 l=1.8u
mp10 NENN BUS LVCC LVCC p w=wp10
mn12 PENN ENB NENN LGND n w=wn10
mn10 PENN BUS LGND LGND n w=wn10
mp11 NENN ENB LVCC LVCC p w=wp11
mp12 NENN ENBN PENN LVCC p w=wp11
mn11 PENN ENBN LGND LGND n w=80u
mp13 ENBN ENB LVCC LVCC p w=35u
mn13 ENBN ENB LGND LGND n w=17u
cbus BUS LGND 1.5pf
cpad OUT LGND 5.0pf
.ends
* * input signals *
482
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
vcc VCC GND 5V
lvcc vcc lvcc 6nh
lgnd lgnd gnd 6nh
vin DATA LGND pl (0v 0n, 5v 0.7n)
vinb DATAbar LGND pl (5v 0n, 0v 0.7n)
ven ENB GND 5V
** circuit **
x1 data out buff
cext1 out GND 50pf
x2 databar outbar buff
cext2 outbar GND 50pf
*Optimization Parameters
.param
+ wp2=opt1(70u,30u,330u)
+ wn2=opt1(22u,15u,400u)
+ wp3=opt1(400u,100u,500u)
+ wn3=opt1(190u,80u,580u)
+ wp4=opt1(670u,150u,800u)
+ wn4=opt1(370u,50u,500u)
+ wp5=opt1(1200u,1000u,5000u)
+ wn5=opt1(600u,400u,2500u)
+ wp10=opt1(240u,150u,450u)
+ wn10=opt1(140u,30u,280u)
+ wp11=opt1(240u,150u,450u)
*Control Section
.tran 1ns 16ns
.tran .5ns 15ns sweep optimize=opt1
+ results=tfopt,tropt,rmspowo model=optmod
** put soft limit for power with minval setting (i.e. values
** less than 1000mw are less important)
.measure rmspowo rms power goal=100mw minval=1000mw
.meas tran tfopt trig v(data) val=2.5 rise=1 targ v(out)
+ val=2.5 fall=1 goal=5.0n
.meas tran tropt trig v(databar) val=2.5 fall=1 targ
+ v(outbar) val=2.5 rise=1 goal=5.0n
.model optmod opt itropt=40 max=1e5 difsiz=1e-5
*.tran 1ns 16ns
* output section *
.probe tran v(data) v(out)
.probe tran v(databar) v(outbar)
*Model Section
HSPICE® Simulation and Analysis User Guide
Y-2006.03
483
Chapter 17: Optimization
Overview
.MODEL N NMOS LEVEL=3 VTO=0.7 UO=500 KAPPA=.25 KP=30U
+ ETA=.03 THETA=.04 VMAX=2E5 NSUB=9E16 TOX=500E-10
+ GAMMA=1.5 PB=0.6 JS=.1M XJ=0.5U LD=0.0 NFS=1E11 NSS=2E10
+ CGSO=200P CGDO=200P CGBO=300P
.MODEL P PMOS LEVEL=3 VTO=-0.8 UO=150 KAPPA=.25 KP=15U
+ ETA=.03 THETA=.04 VMAX=5E4 NSUB=1.8E16 TOX=500E-10
+ NFS=1E11 GAMMA=.672 PB=0.6 JS=.1M XJ=0.5U LD=0.0
+ NSS=2E10 CGSO=200P CGDO=200P CGBO=300P
.end
Figure 69
Tristate Buffer Optimization Circuit
VCC
VCC
VCC
VCC
MP1
DATAN
MP3
MP2
PEN
BUS
MP11
MP10
Cbus
MN1
VCC
VCC
NENN
MN3
MN2
MN12
MP12
VCC
Cext
PENN
Cpad
MP4
MN10
MN11
NEN
MN5
MN4
ENB
VCC
MP13
ENBN
Cenbn
Cenb
MN13
484
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 70
Tristate Input/Output Optimization ACIC2B.TR0 = Before
Optimization, ACIC2B.TR1=Optimized Result
* TRI-STATE I/O OPTIMIZATION
APRIL 22, 2003 5:52:46
5.0
ASIC2.TR1
OUT
4.50
OUTBAR
4.0
ASIC2.TR0
OUT
VOLT [LIN]
3.50
OUTBAR
3.0
2.50
2.0
1.50
1.0
500.0N
0
0
2.0N
4.0N
6.0N
8.0N
TIME [LIN]
10.0N
12.0N
14.0N
15.0N
BJT S Parameters Optimization
The following example optimizes the S parameters to match those specified for
a set of measurements. The .DATA measured in-line data statement contains
these measured S parameters as a function of frequency. The model
parameters of the microwave transistor (LBB, LCC, LEE, TF, CBE, CBC, RB, RE,
RC, and IS) vary. As a result, the measured S parameters (in the .DATA
statement) match the calculated S parameters from the simulation results.
This optimization uses a 2n6604 microwave transistor, and an equivalent circuit
that consists of a BJT, with parasitic resistances and inductances. The BJT is
biased at a 10 mA collector current (0.1 mA base current at DC bias and
bf=100).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
485
Chapter 17: Optimization
Overview
Key HSPICE Features Used
■
.NET command to simulate network analyzer action.
■
.AC optimization.
■
Optimized element and model parameters.
■
Optimizing, compares measured S Parameters to calculated parameters.
■
S Parameters used in magnitude and phase (real and imaginary available).
■
Weighting of data-driven frequency versus S Parameter table. Used for the
phase domain.
Input Netlist File for Optimizing BJT S Parameters
* BJTOPT.SP BJT S PARAMETER OPTIMIZATION
.OPTION ACCT NOMOD POST=2
BJT Equivalent Circuit Input
Use the bjtopt.sp netlist file located in your $<installdir>/demo/hspice/devopt
directory for optimizing BJT S Parameters.
Optimization Results
RESIDUAL SUM OF SQUARES
=5.142639e-02
NORM OF THE GRADIENT
=6.068882e-02
MARQUARDT SCALING PARAMETER=0.340303
CO. OF FUNCTION EVALUATIONS=170
NO. OF ITERATIONS
=35
The maximum number of iterations (25) was exceeded. However, the results
probably are accurate. Increase ITROPT accordingly.
Optimized Parameters OPT1– Final Values
***OPTIMIZED PARAMETERS OPT1 SENS %NORM-SEN
.PARAM LBB = 1.5834N $ 27.3566X 2.4368
.PARAM LCC = 2.1334N $ 12.5835X 1.5138
.PARAM LEE =723.0995P $254.2312X 12.3262
.PARAM TF =12.7611P $ 7.4344G 10.0532
.PARAM CBE =620.5195F $ 23.0855G 1.5300
.PARAM CBC = 1.0263P $346.0167G 44.5016
.PARAM RB
= 2.0582
$ 12.8257M 2.3084
.PARAM RE
=869.8714M $ 66.8123M 4.5597
.PARAM RC =54.2262
$ 3.1427M 20.7359
.PARAM IS =99.9900P $ 3.6533X 34.4463M
486
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 71
BJT-S Parameter Optimization
FILE: BJTOPT.SP NETWORK S-PARAMETER OPTIMIZATION
APRIL 22, 2004 6:22:34
20.0
10.0
1.9879
650.0N
[LIN]
600.0N
550.0N
500.0N
450.0N
400.0N
96.8250N
50.0N
20.0N
100.0X
500.0X
1.08
1.508
2.06
HERTZ [LIN]
BJT Model DC Optimization
The goal is to match forward and reverse Gummel plots obtained from a
HP4145 semiconductor analyzer by using the HSPICE LEVEL=1 GummelPoon BJT model. Because Gummel plots are at low base currents, HSPICE
does not optimize the base resistance. HSPICE also does not optimize forward
and reverse Early voltages (VAF and VAR), because simulation did not
measure VCE data.
The key feature in this optimization is incremental optimization:
1. HSPICE first optimizes the forward-Gummel data points.
2. HSPICE updates forward-optimized parameters into the model.
After updating, you cannot change these parameters.
3. HSPICE next optimizes the reverse-Gummel data points.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
487
Chapter 17: Optimization
Overview
BJT Model DC Optimization Input Netlist File
You can find the sample netlist for this example in the following directory:
$installdir/demo/hspice/devopt/opt_bjt.sp
Figure 72
BJT Optimization Forward Gummel Plots
*FILE: OPT_BJT.SP BJT OPTIMIZATION T2N9547
APRIL 22, 2004 17:42:41
OPT_BJT.SV0
I2IQ1
10.0N
PARIIB
1.0N
I1IQ1
AMP 2 LOW
PARIIC
100.0U
10.0U
1.0U
100.0M
10.0M
1.0M
100.0P
488
400.0M
500.0M
600.0M
BASEF [LIN]
700.0M
800.0M
820.0M
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 73
BJT Optimization Reverse Gummel Plots
*FILE: OPT_BJT.SP BJT OPTIMIZATION T2N9547
APRIL 22, 2004 17:42:41
OPT_BJT.SV1
I2IQ1
10.0N
PARIIB
1.0N
I1IQ1
PARIIC
AMP 2 LCV
100.0U
10.0U
1.0U
100.0M
10.0M
1.0M
100.0P
200.0M
300.0M
400.0M
500.0M
BASER [LIN]
600.0M
700.0M
800.0M
Optimizing GaAsFET Model DC
This example circuit is a high-performance, GaAsFET transistor. The design
target is to match HP4145 DC measured data to the HSPICE LEVEL=3 JFET
model.
The HSPICE strategy is:
■
.MEASURE IDSERR is an ERR1 type function. It provides linear attenuation
of the error results starting at 20 mA. This function ignores all currents below
1 mA. The high-current fit is the most important for this model.
■
The OPT1 function simultaneously optimizes all DC parameters.
■
The .DATA statement merges TD1.dat and TD2.dat data files.
■
The graph plot model sets the MONO=1 parameter to remove the retrace
lines from the family of curves.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
489
Chapter 17: Optimization
Overview
GaAsFET Model DC Optimization Input Netlist File
This example is based on demonstration netlist jopt.sp, which is available in
directory $<installdir>/demo/hspice/devopt:
* file opt_bjt.sp bjt optimization t2n3947
*
* optimize the dc forward and reverse characteristics from a
gummel probe
* all dc gummel-poon dc parameters except base resistance and early
* voltages optimized
*
$..tighten the simulator convergence properties
.option post nomod ingold=2 nopage vntol=1e-10
+ numdgt=5 reli=1e-4 relv=1e-4
$..optimization convergence controls
.model optmod opt relin=1e-4 itropt=30 grad=1e-5 close=10 cut=2
+ cendif=1e-6 relout=1e-4 max=1e6
*****room temp device*******
vber base 0 vbe
vbcr base col vbc
q1 col base 0 bjtmod
$..the model and inital guess
.model bjtmod npn
+ iss = 0. xtf = 1. ns = 1.
+ cjs = 0. vjs = 0.50000 ptf = 0.
+ mjs = 0. eg = 1.10000 af = 1.
+ itf = 0.50000 vtf = 1.00000
+ fc = 0.95000 xcjc = 0.94836
+ subs = 1
+ tf=0.0 tr=0.0 cje=0.0 cjc=0.0 mje=0.5 mjc=0.5 vje=0.6 vjc=0.6
+ rb=0.3 rc=10 vaf=550 var=300
$..these are the optimized parameters
+ bf=bf is=is ikf=ikf ise=ise re=re
+ nf=nf ne=ne
$..these are for reverse base opt
+ br=br ikr=ikr isc=isc
+ nr=nr nc=nc
.param vbe=0 ib=0 ic=0 vce_emit=0 vbc=0 ib_emit=0 ic_emit=0
+ bf= opt1( 100, 50, 350)
+ is= opt1( 5e-15, 5e-16, 1e-13)
+ nf= opt1( 1.0, 0.9, 1.1)
+ ikf=opt1( 50e-3, 1e-3, 1)
+ re= opt1( 10, 0.1, 50)
490
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
+ ise=opt1( 1e-16, 1e-18, 1e-11)
+ ne= opt1( 1.5, 1.2, 2.0)
+
+
+
+
+
br= opt2(
nr= opt2(
ikr=opt2(
isc=opt2(
nc= opt2(
2, 1, 10)
1.0, 0.9, 1.1)
50e-3, 1e-3, 1)
1e-12, 1e-15, 1e-10)
1.5, 1.2, 2.0)
.dc data=basef sweep optimize=opt1 results=ibvbe,icvbe
model=optmod
.meas dc ibvbe err1 par(ib) i2(q1) minval=1e-14 ignore=1e-16
.meas dc icvbe err1 par(ic) i1(q1) minval=1e-14 ignore=1e-16
.dc data=baser sweep optimize=opt2 results=ibvber,icvber
model=optmod
.meas dc ibvber err1 par(ib) i2(q1) minval=1e-14 ignore=1e-16
.meas dc icvber err1 par(ic) i1(q1) minval=1e-14 ignore=1e-16
.dc data=basef
.print dc par(ic) i1(q1) par(ib) i2(q1)
.dc data=baser
.print dc par(ic) i1(q1) par(ib) i2(q1)
.option brief=1
.data basef
vbe vbc ic ib
+ 0.40 0. 1.809e-08 1.793e-10
+ 0.410 0. 2.667e-08 2.546e-10
+ 0.420 0. 3.952e-08 3.640e-10
+ 0.430 0. 5.840e-08 5.198e-10
+ 0.440 0. 8.627e-08 7.487e-10
+ 0.450 0. 1.276e-07 1.082e-09
+ 0.460 0. 1.884e-07 1.564e-09
+ 0.470 0. 2.793e-07 2.278e-09
+ 0.480 0. 4.130e-07 3.318e-09
+ 0.490 0. 6.102e-07 4.836e-09
+ 0.50 0. 9.040e-07 7.083e-09
+ 0.510 0. 1.331e-06 1.033e-08
+ 0.520 0. 1.967e-06 1.514e-08
+ 0.530 0. 2.899e-06 2.219e-08
+ 0.540 0. 4.298e-06 3.261e-08
+ 0.550 0. 6.346e-06 4.786e-08
+ 0.560 0. 9.379e-06 7.036e-08
+ 0.570 0. 1.382e-05 1.034e-07
+ 0.580 0. 2.048e-05 1.522e-07
+ 0.590 0. 3.022e-05 2.236e-07
HSPICE® Simulation and Analysis User Guide
Y-2006.03
491
Chapter 17: Optimization
Overview
+ 0.60 0. 4.463e-05 3.288e-07
+ 0.610 0. 6.586e-05 4.834e-07
+ 0.620 0. 9.735e-05 7.119e-07
+ 0.630 0. 1.430e-04 1.043e-06
+ 0.640 0. 2.105e-04 1.529e-06
+ 0.650 0. 3.104e-04 2.250e-06
+ 0.660 0. 4.564e-04 3.298e-06
+ 0.670 0. 6.681e-04 4.819e-06
+ 0.680 0. 9.806e-04 7.058e-06
+ 0.690 0. 1.429e-03 1.028e-05
+ 0.70 0. 2.075e-03 1.492e-05
+ 0.710 0. 2.984e-03 2.151e-05
+ 0.720 0. 4.250e-03 3.070e-05
+ 0.730 0. 5.971e-03 4.353e-05
+ 0.740 0. 8.297e-03 6.089e-05
+ 0.750 0. 1.127e-02 8.364e-05
+ 0.760 0. 1.493e-02 1.126e-04
+ 0.770 0. 1.918e-02 1.504e-04
+ 0.780 0. 2.378e-02 1.984e-04
+ 0.790 0. 2.864e-02 2.587e-04
+ 0.80 0. 3.383e-02 3.345e-04
+ 0.810 0. 3.929e-02 4.270e-04
+ 0.820 0. 4.504e-02 5.386e-04
.enddata
.data baser
vbc vbe ic ib
+ 0.20 0. -9.170e-10 9.058e-10
+ 0.240 0. -2.700e-09 2.660e-09
+ 0.280 0. -8.681e-09 8.483e-09
+ 0.320 0. -3.072e-08 2.992e-08
+ 0.360 0. -1.177e-07 1.137e-07
+ 0.40 0. -4.708e-07 4.517e-07
+ 0.440 0. -1.848e-06 1.752e-06
+ 0.480 0. -6.574e-06 6.130e-06
+ 0.520 0. -2.088e-05 1.876e-05
+ 0.560 0. -6.245e-05 5.265e-05
+ 0.60 0. -1.823e-04 1.377e-04
+ 0.640 0. -5.194e-04 3.276e-04
+ 0.680 0. -1.467e-03 7.302e-04
+ 0.720 0. -3.969e-03 1.552e-03
+ 0.760 0. -9.658e-03 3.180e-03
+ 0.80 0. -2.050e-02 6.329e-03
.enddata
.end
492
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 74
JFET Optimization
*FILE: JOPT.SP JFET OPTIMIZATION
APRIL 22, 2004 18:41:12
45.0M
40.0M
PARAM [LIN]
35.0M
30.0M
25.0M
20.0M
15.0M
10.0M
5.0M
0
0
1.0
2.0
DESIRED [LIN]
3.0
4.0
Optimizing MOS Op-amp
The design goals for the MOS operational amplifier are:
■
Minimize the gate area (and therefore the total cell area).
■
Minimize the power dissipation.
■
Open-loop transient step response of 100 ns for rising and falling edges.
The HSPICE strategy is:
■
Simultaneously optimize two amplifier cells for rising and falling edges.
■
Total power is power for two cells.
■
The optimization transient analysis must be longer to allow for a range of
values in intermediate results.
■
All transistor widths and lengths are optimized.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
493
Chapter 17: Optimization
Overview
.model mosp pmos (vto=-1 kp=2.4e-5 lambda=.004
+ gamma =.37 tox=3e-8 level=3)
.model mosn nmos (vto=1.2 kp=6.0e-5 lambda=.0004
+ gamma =.37 tox=3e-8 level=3)
.param wm1=opt1(60u,20u,100u)
+ wm5=opt1(40u,20u,100u)
+ wm6=opt1(300u,20u,500u)
+ wm7=opt1(70u,40u,200u)
+ lm=opt1(10u,2u,100u)
+ bias=opt1(2.2,1.2,3.0)
.tran 2.5n 300n sweep optimize=opt1
+ results=delayr,delayf,tot_power,area_min model=opt
.model opt opt itropt=40 close=10 relin=1e-5 relout=1e-5
.tran 2n 150n
.measure delayr trig at=0 targ v(voutr) val=2.5 rise=1 goal=100ns
weight=10
.measure delayf trig at=0 targ v(voutf) val=2.5 fall=1 goal=100ns
weight=10
.measure tot_power avg power goal=10mw weight=5
.measure area_min min par(area) goal=1e-9 minval=100n
.print v(vin+) v(voutr) v(voutf)
.end
HSPICE® Simulation and Analysis User Guide
Y-2006.03
495
Chapter 17: Optimization
Overview
Figure 75
CMOS Op-amp
vsupply
M4
M3
M6
vout
vin-
M1
vbias
496
M2
vin+
M5
M7
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 17: Optimization
Overview
Figure 76
Operational Amplifier Optimization
AMPORT.SP MOS OPERATIONAL AMPLIFIER OPTIMIZATION
APRIL 22, 2004 18:57:06
3.9877
3.0
VOLT [LIN]
2.0
1.0
6.40M
6.20M
6.0M
5.80M
5.60M
5.40M
0
25.0N
50.0N
75.0N
100.0N
125.0N
150.0N
TIME [LIN]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
497
Chapter 17: Optimization
Overview
498
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 18: RC Reduction
Linear Acceleration
18
18
RC Reduction
Describes RC network reduction.
Linear Acceleration
Linear acceleration, by using the SIM_LA option, accelerates the simulation of
circuits that include large linear RC networks. To achieve this acceleration,
HSPICE linearly reduces all matrices that represent RC networks. The result is
a smaller matrix that maintains the original port behavior, yet achieves
significant savings in memory and computation. Thus, the SIM_LA option is
ideal for circuits with large numbers of resistors and capacitors, such as clock
trees, power lines, or substrate networks.
In general, the RC elements are separated into their own network. The nodes
shared by both main circuit elements (including .PRINT, .PROBE,
and .MEASURE statements), and RC elements are the port nodes of the RC
network,. All other RC nodes are internal nodes. The currents flowing into the
port nodes are a frequency-dependent function of the voltages at those nodes.
The multiport admittance of a network represents this relationship.
■
The SIM_LA option formulates matrices to represent multiport admittance.
■
Then, to eliminate as many internal nodes as possible, it reduces the size of
these matrices, while preserving the admittance, otherwise known as port
node behavior.
■
The amount of reduction depends on the f0 upper frequency, the threshold
frequency where SIM_LA preserves the admittance. This is shown
graphically in Figure 77.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
499
Chapter 18: RC Reduction
Linear Acceleration
Multiport Admittance vs. Frequency
nce
itta
m
d
a
ual
approx
act
admittance
Figure 77
f0
frequency
The SIM_LA option is very effective for post-layout simulation, because of the
volume of parasitics. For frequencies below f0, the approx signal matches that
of the original admittance. Above f0, the two waveforms diverge, but
presumably the higher frequencies are not of interest. The lower the f0
frequency, the greater the amount of reduction.
For the syntax and description of this control option, see .OPTION SIM_LA in
the HSPICE Command Reference.
You can choose one of two algorithms, explained in the following sections:
■
PACT Algorithm
■
PI Algorithm
PACT Algorithm
The PACT (Pole Analysis via Congruence Transforms) algorithm reduces the
RC networks in a well-conditioned manner, while preserving network stability.
■
The transform preserves the first two moments of admittance at DC (slope
and offset), so that DC behavior is correct (see Figure 78).
■
The algorithm preserves enough low-frequency poles from the original
network to maintain the circuit behavior up to a specified maximum
frequency f0, within the specified tolerance.
This approach is more accurate between these two algorithms, and is the
default.
500
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 18: RC Reduction
Linear Acceleration Control Options Summary
PACT Algorithm
ed
erv
s
re
tp
e
s
off
nd
ce
a
tan
e
t
i
p
dm
slo
al a
u
t
ac
admittance
Figure 78
PACT: poles added
f0
frequency
PI Algorithm
This algorithm creates a pi model of the RC network.
■
For a two-port, the pi model reduced network consists of:
•
a resistor connecting the two ports, and
•
a capacitor connecting each port to ground
The result resembles the Greek letter pi.
■
For a general multiport, SIM_LA preserves the DC admittance between the
ports, and the total capacitance that connects the ports to ground. All
floating capacitances are lumped to ground.
Linear Acceleration Control Options Summary
In addition to SIM_LA, other options are available to control the maximum
resistance and minimum capacitance values to preserve, and to limit the
operating parameters of the PACT algorithm. Table 56 contains a summary of
HSPICE® Simulation and Analysis User Guide
Y-2006.03
501
Chapter 18: RC Reduction
Linear Acceleration Control Options Summary
these control options. For their syntax and descriptions, see the respective
section in the HSPICE Command Reference.
Table 56
PACT Options
Syntax
Description
.OPTION SIM_LA=PACT | PI
Activates linear matrix reduction and selects between two
methods. For HSPICE RF, if you set the entire netlist to
ANALOG mode, linear matrix reduction does not occur.
.OPTION LA_FREQ=<value>
Upper frequency where you need accuracy preserved. value
is the upper frequency for which the PACT algorithm
preserves accuracy. If value is 0, PACT drops all capacitors,
because only DC is of interest. The maximum frequency
required for accurate reduction depends on both the
technology of the circuit and the time scale of interest. In
general, the faster the circuit, the higher the maximum
frequency. The default is 1GHz.
.OPTION LA_MAXR=<value>
Maximum resistance for linear matrix reduction. value is the
maximum resistance preserved in the reduction. SIM_LA
assumes that any resistor greater than value has an infinite
resistance, and drops the resistor after reduction finishes. The
default is 1e15 ohms.
.OPTION LA_MINC=<value>
Minimum capacitance for linear matrix reduction. value is the
minimum capacitance preserved in the reduction. After
reduction completes, SIM_LA lumps any capacitor smaller
than value to ground. The default is 1e-16 farads.
.OPTION LA_TIME=<value>
Minimum time for which accuracy must be preserved. value is
the minimum switching time for which the PACT algorithm
preserves accuracy. HSPICE does not accurately represent
waveforms that occur more rapidly than this time. LA_TIME is
simply the dual of LA_FREQ. The default is 1ns, equivalent to
setting LA_FREQ=1GHz.
.OPTION LA_TOL=<value>
Error tolerance for the PACT algorithm. value is the error
tolerance for the PACT algorithm, is between 0.0 and 1.0. The
default is 0.05.
502
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 18: RC Reduction
Linear Acceleration Control Options Summary
Example
In this example, the circuit has a typical risetime of 1ns. Set the maximum
frequency to 1 GHz, or set the minimum switching time to 1ns.
.OPTION LA_FREQ = 1GHz
-or.OPTION LA_TIME = 1ns
However, if spikes occur in 0.1ns, HSPICE will not accurately simulate them. To
capture the behavior of the spikes, use:
.OPTION LA_FREQ = 10GHz
-or.OPTION LA_TIME = 0.1ns
Note:
Higher frequencies (smaller times) increase accuracy, but only up to the
minimum time step used in HSPICE.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
503
Chapter 18: RC Reduction
Linear Acceleration Control Options Summary
504
HSPICE® Simulation and Analysis User Guide
Y-2006.03
19
Running Demonstration Files
19
Contains examples of basic file construction techniques, advanced features,
and simulation tricks. Lists and describes several HSPICE and HSPICE RF
input files.
Using the Demo Directory Tree
Demonstration Input Files on page 524 lists demonstration files, which are
designed as good training examples. Most HSPICE or HSPICE RF distributions
include these examples in the demo directory tree, where $installdir is
the installation directory environment variable:
Table 57
Directory
File
Description
$installdir/demo/hspice
/alge
algebraic output
/apps
general applications
/behave
analog behavioral components
/bench
standard benchmarks
/bjt
bipolar components
/cchar
characteristics of cell prototypes
/ciropt
circuit level optimization
/ddl
Discrete Device Library
/devopt
device level optimization
HSPICE® Simulation and Analysis User Guide
Y-2006.03
505
Chapter 19: Running Demonstration Files
Two-Bit Adder Demo
Table 57
Directory
File
Description
/fft
Fourier analysis (HSPICE only)
/filters
filters
/mag
transformers, magnetic core components
/mos
MOS components
/rad
radiation effects (photocurrent)
/sources
dependent and independent sources
/tline
filters and transmission lines
/veriloga
Verilog-A examples
Two-Bit Adder Demo
This two-bit adder shows how to improve efficiency, accuracy, and productivity
in circuit simulation. The adder is in the $installdir/demo/hspice/apps/
mos2bit.sp (or $installdir/demo/hspicext/apps/mos2bit.sp for HSPICE RF)
demonstration file. It consists of two-input NAND gates, defined using the
NAND sub-circuit. CMOS devices include length, width, and output loading
parameters. Descriptive names enhance the readability of this circuit.
One-Bit Subcircuit
The ONEBIT subcircuit defines the two half adders, with carry in and carry out.
To create the two-bit adder, HSPICE or HSPICE RF uses two calls to ONEBIT.
Independent piecewise linear voltage sources provide the input stimuli. The R
repeat function creates complex waveforms.
506
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Two-Bit Adder Demo
Figure 79
One-bit Adder sub-circuit
1
in1
X8
X2
in2
X4
X7
10
13
X5
X1
half1
2
9
X6
half2
carry-out
#1_nand
X9
Two-bit Adder Circuit
A(0)
carry-in
out
4
TIME [LIN]
X3
carry-in
Figure 80
X8
B(0)
A(1)
B(1)
carry-out_1
One Bit
One Bit
C(0)
C(1)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
carry-out_2
507
Chapter 19: Running Demonstration Files
MOS I-V and C-V Plotting Demo
Figure 81
in1
1-bit NAND Gate Binary Adder
1
X8
X2
in2
X4
X7
10
13
X5
X1
half1
2
X8
4
TIME [LIN]
X3
out
9
carry-in
X6
half2
carry-out
#1_nand
X9
MOS Two-Bit Adder Input File
You can find the sample netlist for this example in the following directory:
$installdir/demo/hspice/apps/mos2bit.sp
MOS I-V and C-V Plotting Demo
To diagnose a simulation or modeling problem, you usually need to review the
basic characteristics of the transistors. You can use this demonstration
template file, $installdir/demo/hspice/mos/mosivcv.sp (or $installdir/demo/
hspicext/mos/mosivcv.sp for HSPICE RF), with any MOS model. The example
shows how to easily create input files, and how to display the complete
graphical results. The following features aid model evaluations:
Table 58
508
MOS I-V and C-V Plotting Demo
Value
Description
SCALE=1u
Sets the element units to microns (not meters). Most circuit
designs use microns.
DCCAP
Forces HSPICE or HSPICE RF to evaluate the voltage variable
capacitors, during a DC sweep.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
MOS I-V and C-V Plotting Demo
Table 58
MOS I-V and C-V Plotting Demo
Value
Description
node names
Makes a circuit easy to understand. Symbolic name contains up to
16 characters.
.GRAPH
.GRAPH statements create high-resolution plots. To set additional
characteristics, add a graph model.
Plotting Variables
Use this template to plot internal variables, such as:
Table 59
Demo Plotting Variables
Variable
Description
i(mn1)
i1, i2, i3, or i4 can specify the true branch currents for each transistor
node.
LV18(mn6)
Total gate capacitance (C-V plot).
LX7(mn1)
GM gate transconductance. (LX8 specifies GDS, and LX9 specifies
GMB).
HSPICE® Simulation and Analysis User Guide
Y-2006.03
509
Chapter 19: Running Demonstration Files
MOS I-V and C-V Plotting Demo
Figure 82
MOS IDS Plot
*FILE: MOS2BJT.SP TR0 BJT MOS ADDER
APRIL 24, 2003 13:12:24
4.50
4.0
MOS2BJT.TR0
3.50
VOLT [LIN]
VOLT [LIN]
3.0
2.50
2.0
1.50
1.0
500.0M
0
0
10.0N
20.0N
30.0N
40.0N
50.0N
60.0N
TIME [LIN]
510
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
MOS I-V and C-V Plotting Demo
Figure 83
MOS VGS Plot
*FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOT
APRIL 24, 2003 14:18:58
200.0U
180.0U
160.0U
AMP [LIN]
140.0U
120.0U
100.0U
80.0U
60.0U
40.0U
20.0U
0
0
1.0
2.0
3.0
VOLTS [LIN]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
4.0
5.0
511
Chapter 19: Running Demonstration Files
MOS I-V and C-V Plotting Demo
Figure 84
MOS GM Plot
*FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS
APRIL 24, 2003 14:31:48
59.5887U
55.0U
50.0U
45.0U
AMP [LIN]
40.0U
35.0U
30.0U
25.0U
20.0U
15.0U
10.0U
5.0U
0
512
0
1.0
2.0
3.0
VOLTS [LIN]
4.0
5.0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
CMOS Output Driver Demo
Figure 85
MOS C-V Plot
*FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS
APRIL 24, 2003 14:42:16
13.7840F
13.0F
12.0F
LX [LIN]
11.0F
10.0F
9.0F
8.0F
7.0F
6.0F
0
1.0
2.0
3.0
VOLTS [LIN]
4.0
5.0
MOS I-V and C-V Plot Example Input File
You can find the sample netlist for this example in the following directory:
$installdir/demo/hspice/mos/mosivcv.sp
CMOS Output Driver Demo
ASIC designers need to integrate high-performance IC parts onto a printed
circuit board (PCB). The output driver circuit is critical to system performance.
The $installdir/demo/hspice/apps/asic1.sp (or $installdir/demo/hspicext/apps/
asic1.sp for HSPICE RF) demonstration file shows models for an output driver,
the bond wire and leadframe, and a six-inch length of copper transmission line.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
513
Chapter 19: Running Demonstration Files
CMOS Output Driver Demo
This simulation demonstrates how to:
■
Define parameters, and measure test outputs.
■
Use the LUMP5 macro to input geometric units, and convert them to
electrical units.
■
Use .MEASURE statements to calculate the peak local supply current,
voltage drop, and power.
■
Measure RMS power, delay, rise times, and fall times.
■
Simulate and measure an output driver under load. The load consists of:
•
Bondwire and leadframe inductance.
•
Bondwire and leadframe resistance.
•
Leadframe capacitance.
•
Six inches of 6-mil copper, on an FR-4 printed circuit board.
•
Capacitive load, at the end of the copper wire.
Strategy
The HSPICE or HSPICE RF strategy is to:
514
■
Create a five-lump transmission line model for the copper wire.
■
Create single lumped models for leadframe loads.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
CMOS Output Driver Demo
Figure 86
Noise Bounce
*FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS
APRIL 24, 2004 14:53:29
59.5887U
55.0U
50.0U
45.0U
LX [LIN]
40.0U
35.0U
30.0U
25.0U
20.0U
15.0U
10.0U
5.0U
0
0
1.0
2.0
3.0
4.0
5.0
VOLTS [LIN]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
515
Chapter 19: Running Demonstration Files
CMOS Output Driver Demo
Figure 87
Asic1.sp Demo Local Supply Voltage
*FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS
APRIL 24, 2003 15:24:31
13.7840F
13.0F
LX [LIN]
12.0F
11.0F
10.0F
9.0F
8.0F
7.0F
6.0F
0
516
1.0
2.0
3.0
VOLTS [LIN]
4.0
5.0
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
CMOS Output Driver Demo
Figure 88
5.8829
Asic1.sp Demo Local Supply Current
*FILE: ASIC1.SP GROUND BOUNCE FOR I/O CMOS DRIVER
APRIL 24, 2003 15:29:24
5.0
LX [LIN]
4.0
3.0
2.0
1.0
0
-1.0
0
5.0N
10.0N
15.0N
20.0N
25.0N
30.0N
TIME [LIN]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
517
Chapter 19: Running Demonstration Files
Temperature Coefficients Demo
Figure 89
Asic1.sp Demo Input and Output Signals
*FILE: ASIC1.SP GROUND BOUNCE FOR I/O CMOS DRIVER
APRIL 24, 2004 15:39:18
325.0M
300.0M
275.0M
PARAM [LIN]
250.0M
225.0M
200.0M
175.0M
150.0M
125.0M
100.0M
75.0M
50.0M
25.0M
0
5.0N
10.0N
15.0N
TIME [LIN]
20.0N
25.0N
30.0N
CMOS Output Driver Example Input File
You can find the sample netlist for this example in the following directory:
$installdir/demo/hspice/apps/asic1.sp
Temperature Coefficients Demo
SPICE-type simulators do not always automatically compensate for variations
in temperature. The simulators make many assumptions that are not valid for
all technologies. Many of the critical model parameters in HSPICE or HSPICE
RF provide first-order and second-order temperature coefficients, to ensure
accurate simulations.
518
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Temperature Coefficients Demo
You can optimize these temperature coefficients in either of two ways.
■
The first method uses the TEMP DC sweep variable.
All analysis sweeps allow two sweep variables. To optimize the temperature
coefficients, one of these must be the optimize variable. Sweeping TEMP
limits the component to a linear element, such as a resistor, inductor, or
capacitor.
■
The second method uses multiple components at different temperatures.
Example
The following example, the $installdir/demo/hspice/ciropt/opttemp.sp (or
$installdir/demo/hspicext/ciropt/opttemp.sp for HSPICE RF) demo file,
simulates three circuits of a voltage source. It also simulates a resistor at -25, 0,
and +25°C from nominal, using the DTEMP parameter for element delta
temperatures. The resistors share a common model.
You need three temperatures to solve a second-order equation. You can extend
this simulation template to a transient simulation of non-linear components
(such as bipolar transistors, diodes, and FETs).
This example uses some simulation shortcuts. In the internal output templates
for resistors, LV1 (resistor) is the conductance (reciprocal resistance) at the
desired temperature.
■
You can run optimization in the resistance domain.
■
To optimize more complex elements, use the current or voltage domain, with
measured sweep data.
The error function expects a sweep on at least two points, so the data
statement must include two duplicate points.
Input File for Optimized Temperature Coefficients
You can find the sample netlist for this example in the following directory:
$installdir/demo/hspice/ciropt/opttemp.sp
HSPICE® Simulation and Analysis User Guide
Y-2006.03
519
Chapter 19: Running Demonstration Files
Simulating Electrical Measurements
Optimization Section
.model optmod opt
.dc data=RES_TEMP optimize=opt1
+
[email protected],[email protected],[email protected]
+
model=optmod
.param tc1r_opt=opt1(.001,-.1,.1)
.param tc2r_opt=opt1(1u,-1m,1m)
.meas [email protected] err2 par(R_meas_t1) par('1.0 / lv1(r-25)')
.meas [email protected] err2 par(R_meas_t2) par('1.0 / lv1(r0) ')
.meas [email protected] err2 par(R_meas_t3) par('1.0 / lv1(r+25) ')
* * Output section *
.dc data=RES_TEMP
.print 'r1_diff'=par('1.0/lv1(r-25)')
+
'r2_diff'=par('1.0/lv1(r0) ')
+
'r3_diff'=par('1.0/lv1(r+25)')
.data RES_TEMP R_meas_t1 R_meas_t2 R_meas_t3
950 1000 1010
950 1000 1010
.enddata
.end
Simulating Electrical Measurements
In this example, HSPICE or HSPICE RF simulates electrical measurements,
which return device characteristics for data sheets. The demonstration file for
this example is $installdir/demo/hspice/ddl/t2n2222.sp (or $installdir/demo/
hspicext/ddl/t2n2222.sp for HSPICE RF). This example automatically includes
DDL models by reference, using either the DDLPATH environment variable, or
the .OPTION SEARCH=path statement. It also combines an AC circuit and
measurement, with a transient circuit and measurement.
The AC circuit measures the maximum Hfe, which is the small-signal common
emitter gain. HSPICE or HSPICE RF uses the .MEASURE WHEN statement to
calculate the unity gain frequency, and the phase at the specified frequency. In
the Transient Measurements section of the input file, a segmented transient
statement speeds-up simulation, and compresses the output graph.
Measurements include:
520
■
TURN ON from 90% of input rising, to 90% of output falling.
■
OUTPUT FALL from 90% to 10% of output falling.
■
TURN OFF from 10% of input falling, to 10% of output rising.
■
OUTPUT RISE from 10% to 90% of output rising.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Modeling Wide-Channel MOS Transistors
Figure 90
T2N2222 Optimization
*FILE: ASIC2.SP TEST OF I/O STAGE LUMPED MOS MODEL
APRIL 24, 2003 15:52:09
10.0M
9.0M
8.0M
7.0M
PARAM (LIN)
6.0M
5.0M
4.0M
3.0M
2.0M
1.0M
0
-1.0M 0
200.0P
400.0P
600.0P
800.0P
TIME [LIN]
T2N2222 Optimization Example Input File
You can find the sample netlist for this example in the following directory:
$installdir/demo/hspice/ddl/t2n2222.sp
Modeling Wide-Channel MOS Transistors
If you select an appropriate model for I/O cell transistors, simulation accuracy
improves. For wide-channel devices, model the transistor as a group of
transistors, connected in parallel, with appropriate RC delay networks. If you
model the device as only one transistor, the polysilicon gate introduces delay.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
521
Chapter 19: Running Demonstration Files
Modeling Wide-Channel MOS Transistors
When you scale to higher-speed technologies, the area of the polysilicon gate
decreases, reducing the gate capacitance. However, if you scale the gate oxide
thickness, the capacitance per unit area increases, which also increases the
RC product.
Example
The following example illustrates how scaling affects the delay. For example, for
a device with:
■
Channel width=100 microns.
■
Channel length=5 microns.
■
Gate oxide thickness=800 Angstroms.
The resulting RC product for the polysilicon gate is:
W
Rpoly = ----- ⋅ 40
L
Esio ⋅ nsi
poly = ----------------------- ⋅ L ⋅ W
tox
100
Rpoly = --------- ⋅ 40 = 800 ,
5
3.9 ⋅ 8.86
Co = ---------------------- ⋅ 100 ⋅ 5 = 215 fF RC=138 ps
800
For a transistor with:
■
Channel width=100 microns.
■
Channel length=1.2 microns.
■
Gate oxide thickness=250 Angstroms.
The resulting RC product for the polysilicon gate is:
channel width
Rpoly = ----------------------------------------- ⋅ 40
channel length
3.9 ⋅ 8.86
Co = ---------------------- ⋅ channel width ⋅ channel length RC=546 ps
Tox
You can use a nine-stage ladder model to model the RC delay in CMOS
devices.
522
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Modeling Wide-Channel MOS Transistors
Figure 91
Nine-stage Ladder Model
Drain
M1
W/18
M2
W/9
M3
W/9
M4
W/9
M5
W/19
M6
W/9
M7
W/9
M8
W/9
M9
W/9
M10
W/18
Bulk Source
In this example, the nine-stage ladder model is in data file $installdir/demo/
hspice/apps /asic3.sp. To optimize this model, HSPICE uses measured data
from a wide channel transistor as the target data\. Optimization produces a
nine-stage ladder model, which matches the timing characteristics of the
physical data (HSPICE RF does not support optimization). HSPICE compares
the simulation results for the nine-stage ladder model, and the one-stage model
by using the nine-stage ladder model as the reference. The one-stage model
results are about 10% faster than actual physical data indicates.
Example
You can find the sample Nine-Stage Ladder model netlist for this example in the
following directory:
$installdir/demo/hspice/apps/asic3.sp
HSPICE® Simulation and Analysis User Guide
Y-2006.03
523
Chapter 19: Running Demonstration Files
Demonstration Input Files
Figure 92
Asic3 Single vs. Lumped Model
*FILE: ASIC2.SP TEST OF I/O STAGE LUMPED MOS MODEL
APRIL 24, 2004 16:02:35
10.0M
9.0M
8.0M
PARAM [LIN]
7.0M
6.0M
5.0M
4.0M
3.0M
2.0M
1.0M
0
-1.0M
0
200.0
400.0
TIME [LIN]
600.0
800.0
Demonstration Input Files
File Name
Description
Algebraic Output Variable Examples $installdir/demo/hspice/alge
524
alg.sp
demonstrates algebraic parameters
alg_fil.sp
magnitude response of the behavioral filter model
alg_vco.sp
voltage-controlled oscillator
alg_vf.sp
voltage-to-frequency converter behavioral model
xalg1.sp
QA of parameters
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
xalg2.sp
QA of parameters
Applications of General Interest $installdir/demo/hspice/apps
alm124.sp
AC, noise, and transient op-amp analysis
alter2.sp
.ALTER examples
ampg.sp
pole/zero analysis of a G source amplifier
asic1.sp
ground bounce for I/O CMOS driver
asic3.sp
ten-stage lumped MOS model
bjt2bit.sp
BJT two-bit adder
bjt4bit.sp
four-bit all NAND gate, binary adder
bjtdiff.sp
BJT diff amp with every analysis type
bjtschmt.sp
bipolar Schmidt trigger
bjtsense.sp
bipolar sense amplifier
cellchar.sp
characteristics of ASIC inverter cell
crystal.sp
crystal oscillator circuit
gaasamp.sp
simple GaAsFET amplifier
grouptim.sp
group time-delay example
inv.sp
sweep MOSFET -3 sigma to +3 sigma use .MEASURE output
mcdiff.sp
CMOS differential amplifier
mondc_a.sp
Monte Carlo of MOS diffusion and photolithographic effects
(HSPICE only)
mondc_b.sp
Monte Carlo DC analysis (HSPICE only)
mont1.sp
Monte Carlo Gaussian, uniform, and limit function (HSPICE only)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
525
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
mos2bit.sp
two-bit MOS adder
opampdcm.sp
DCmatch analysis
pll.sp
phase-locked loop
sclopass.sp
switched-capacitor low-pass filter
worst.sp
worst case skew models by using .ALTER
xbjt2bit.sp
BJT NAND gate two-bit binary adder
Behavioral Applications $installdir/demo/hspice/behave
526
acl.sp
acl gate
amp_mod.sp
amplitude modulator with pulse waveform carrier
behave.sp
AND/NAND gates by using G, E Elements
calg2.sp
voltage variable capacitance
det_dff.sp
double edge-triggered flip-flop
diff.sp
differentiator circuit
diode.sp
behavioral diode by using a PWL VCCS
dlatch.sp
CMOS D-latch by using behaviorals
galg1.sp
sampling a sine wave
idealop.sp
ninth-order low-pass filter
integ.sp
integrator circuit
invb_op.sp
optimizes the CMOS macromodel inverter
ivx.sp
characteristics of the PMOS and NMOS as a switch
op_amp.sp
op-amp from Chua and Lin
pd.sp
phase detector modeled as switches
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
pdb.sp
phase detector by using behavioral NAND gates
pwl10.sp
operational amplifier used as a voltage follower
pwl2.sp
PPW-VCCS with a gain of 1 amp/volt
pwl4.sp
eight-input NAND gate
pwl7.sp
modeling inverter by using a PWL VCVS
pwl8.sp
smoothing the triangle waveform by using the PWL CCCS
ring5bm.sp
five-stage ring oscillator – macromodel CMOS inverter
ringb.sp
ring oscillator by using behavioral model
sampling.sp
sampling a sine wave
scr.sp
silicon-controlled rectifier, modeled using the PWL CCVS
swcap5.sp
fifth-order elliptic switched capacitor filter
switch.sp
test for PWL switch element
swrc.sp
switched capacitor RC circuit
triode.sp
triode model family of curves by using behavioral elements
triodex.sp
triode model family of curves by using behavioral elements
tunnel.sp
modeling tunnel diode characteristic by using PWL VCCS
vcob.sp
voltage-controlled oscillator by using PWL functions
Benchmarks $installdir/demo/hspice/bench
bigmos1.sp
large MOS simulation
demo.sp
quick demo file to test installation
m2bit.sp
72-transistor two-bit adder – typical cell simulation
m2bitf.sp
fast simulation example
HSPICE® Simulation and Analysis User Guide
Y-2006.03
527
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
m2bitsw.sp
Fast simulation example. Same as m2bitf.sp, but uses behavioral
elements
senseamp.sp
bipolar analog test case
Timing Analysis $installdir/demo/hspice/bisect
fig3a.sp
DFF bisection search for setup time
fig3b.sp
DFF early, optimum, and late setup times
inv_a.sp
inverter bisection (pass-fail)
BJT and Diode Devices $installdir/demo/hspice/bjt
bjtbeta.sp
plot BJT beta
bjtft.sp
plot BJT FT by using s-parameters
bjtgm.sp
plot BJT Gm, Gpi
dpntun.sp
junction tunnel diode
snaphsp.sp
convert SNAP to HSPICE
tun.sp
tunnel oxide diode
Cell Characterization $installdir/demo/hspice/cchar
528
dff.sp
DFF bisection search for setup time
inv3.sp
characteristics of an inverter
inva.sp
characteristics of an inverter
invb.sp
characteristics of an inverter
load1.sp
inverter sweep, delay versus fanout
setupbsc.sp
setup characteristics
setupold.sp
setup characteristics
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
setuppas.sp
setup characteristics
sigma.sp
sweep MOSFET -3 sigma to +3 sigma by using measure output
tdgtl.a2d
Viewsim A2D HSPICE or HSPICE RF input file
tdgtl.d2a
Viewsim D2A HSPICE or HSPICE RF input file
tdgtl.sp
two-bit adder by using D2A Elements
Circuit Optimization $installdir/demo/hspice/ciropt
ampgain.sp
set unity gain frequency of a BJT diff pair
ampopt.sp
optimize area, power, speed of a MOS amp
asic2.sp
optimize speed, power of a CMOS output buffer
asic6.sp
find best width of a CMOS input buffer
delayopt.sp
optimize group delay of an LCR circuit
lpopt.sp
match lossy filter to ideal filter
opttemp.sp
find first and second temperature coefficients of a resistor
rcopt.sp
optimize speed or power for an RC circuit
DDL $installdir/demo/hspice/ddl
ad8bit.sp
eight-bit A/D flash converter
alf155.sp
characteristics of National JFET op-amp
alf156.sp
characteristics of National JFET op-amp
alf157.sp
characteristics of National JFET op-amp
alf255.sp
characteristics of National JFET op-amp
alf347.sp
characteristics of National JFET op-amp
alf351.sp
characteristics of National wide-bandwidth, JFET input, op-amp
HSPICE® Simulation and Analysis User Guide
Y-2006.03
529
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
alf353.sp
characteristics of National wide-bandwidth, dual JFET input, op-amp
alf355.sp
characteristics of Motorola JFET, op-amp
alf356.sp
characteristics of Motorola JFET, op-amp
alf357.sp
characteristics of Motorola JFET, op-amp
alf3741.sp
alm101a.sp
530
alm107.sp
characteristics of National op-amp
alm108.sp
characteristics of National op-amp
alm108a.sp
characteristics of National op-amp
alm118.sp
characteristics of National op-amp
alm124.sp
characteristics of National low-power, quad op-amp
alm124a.sp
characteristics of National low-power, quad op-amp
alm158.sp
characteristics of National op-amp
alm158a.sp
characteristics of National op-amp
alm201.sp
characteristics of LM201 op-amp
alm201a.sp
characteristics of LM201 op-amp
alm207.sp
characteristics of National op-amp
alm208.sp
characteristics of National op-amp
alm208a.sp
characteristics of National op-amp
alm224.sp
characteristics of National op-amp
alm258.sp
characteristics of National op-amp
alm258a.sp
characteristics of National op-amp
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
alm301a.sp
characteristics of National op-amp
alm307.sp
characteristics of National op-amp
alm308.sp
characteristics of National op-amp
alm308a.sp
characteristics of National op-amp
alm318.sp
characteristics of National op-amp
alm324.sp
characteristics of National op-amp
alm358.sp
characteristics of National op-amp
alm358a.sp
characteristics of National op-amp
alm725.sp
characteristics of National op-amp
alm741.sp
characteristics of National op-amp
alm747.sp
characteristics of National op-amp
alm747c.sp
characteristics of National op-amp
alm1458.sp
characteristics of National dual op-amp
alm1558.sp
characteristics of National dual op-amp
alm2902.sp
characteristics of National op-amp
alm2904.sp
characteristics of National op-amp
amc1458.sp
characteristics of Motorola internally-compensated, highperformance op-amp
amc1536.sp
characteristics of Motorola internally-compensated, high-voltage opamp
amc1741.sp
characteristics of Motorola internally-compensated, highperformance op-amp
amc1747.sp
characteristics of Motorola internally-compensated, highperformance op-amp
HSPICE® Simulation and Analysis User Guide
Y-2006.03
531
Chapter 19: Running Demonstration Files
Demonstration Input Files
532
File Name
Description
ane5534.sp
characteristics of TI low-noise, high-speed op-amp
anjm4558.sp
characteristics of TI dual op-amp
anjm4559.sp
characteristics of TI dual op-amp
anjm4560.sp
characteristics of TI dual op-amp
aop04.sp
characteristics of PMI op-amp
aop07.sp
characteristics of PMI ultra-low offset voltage, op-amp
aop14.sp
characteristics of PMI op-amp
aop15b.sp
characteristics of PMI precision JFET input, op-amp
aop16b.sp
characteristics of PMI precision JFET input, op-amp
at094cns.sp
characteristics of TI op-amp
atl071c.sp
characteristics of TI low-noise, op-amp
atl072c.sp
characteristics of TI low-noise, op-amp
atl074c.sp
characteristics of TI low-noise, op-amp
atl081c.sp
characteristics of TI JFET op-amp
atl082c.sp
characteristics of TI JFET op-amp
atl084c.sp
characteristics of TI JFET op-amp
atl092cp.sp
characteristics of TI op-amp
atl094cn.sp
characteristics of TI op-amp
aupc358.sp
characteristics of NEC general, dual op-amp
aupc1251.sp
characteristics of NEC general, dual op-amp
j2n3330.sp
characteristics of JFET 2n3330 I-V
mirf340.sp
characteristics of IRF340 I-V
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
t2n2222.sp
characteristics of BJT 2n2222
Device Optimization (HSPICE only) $installdir/demo/hspice/devopt
beta.sp
LEVEL=2 beta optimization
bjtopt.sp
s-parameter optimization of a 2n6604 BJT
bjtopt1.sp
2n2222 DC optimization
bjtopt2.sp
2n2222 Hfe optimization
d.sp
diode, multiple temperatures
dcopt1.sp
1n3019 diode, I-V and C-V optimization
gaas.sp
JFET optimization
jopt.sp
300u/1u GaAs FET, DC optimization
jopt2.sp
JFET optimization
joptac.sp
300u/1u GaAs FET, 40 MHz–20 GHz, s-parameter optimization
l3.sp
MOS LEVEL 3 optimization
l3a.sp
MOS LEVEL 3 optimization
l28.sp
LEVEL=28 optimization
ml2opt.sp
MOS LEVEL=2 I-V optimization
ml3opt.sp
MOS LEVEL=3 I-V optimization
ml6opt.sp
MOS LEVEL=6 I-V optimization
ml13opt.sp
MOS LEVEL=13 I-V optimization
opt_bjt.sp
2n3947 forward and reverse Gummel optimization
Fourier Analysis (HSPICE only) $installdir/demo/hspice/fft
am.sp
FFT analysis, AM source
HSPICE® Simulation and Analysis User Guide
Y-2006.03
533
Chapter 19: Running Demonstration Files
Demonstration Input Files
534
File Name
Description
bart.sp
FFT analysis, Bartlett window
black.sp
FFT analysis, Blackman window
dist.sp
FFT analysis, second harmonic distortion
exam1.sp
FFT analysis, AM source
exam3.sp
FFT analysis, high-frequency signal detection test
exam4.sp
FFT analysis, small-signal harmonic distortion test
exp.sp
FFT analysis, exponential source
fft.sp
FFT analysis, transient, sweeping a resistor
fft1.sp
FFT analysis, transient
fft2.sp
FFT analysis on the product of three waveforms
fft3.sp
FFT analysis, transient, sweeping frequency
fft4.sp
FFT analysis, transient, Monte Carlo Gaussian distribution
fft5.sp
FFT analysis, data-driven transient analysis
fft6.sp
FFT analysis, sinusoidal source
gauss.sp
FFT analysis, Gaussian window
hamm.sp
FFT analysis, Hamming window
hann.sp
FFT analysis, Hanning window
harris.sp
FFT analysis, Blackman-Harris window
intermod.sp
FFT analysis, intermodulation distortion
kaiser.sp
FFT analysis, Kaiser window
mod.sp
FFT analysis, modulated pulse
pulse.sp
FFT analysis, pulse source
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
pwl.sp
FFT analysis, piecewise linear source
rect.sp
FFT analysis, rectangular window
rectan.sp
FFT analysis, rectangular window
sffm.sp
FFT analysis, single-frequency FM source
sine.sp
FFT analysis, sinusoidal source
swcap5.sp
FFT analysis, fifth-order elliptic, switched-capacitor filter
tri.sp
FFT analysis, rectangular window
win.sp
FFT analysis, window test
window.sp
FFT analysis, window test
winreal.sp
FFT analysis, window test
Filters $installdir/demo/hspice/filters
fbp_1.sp
bandpass LCR filter, measurement
fbp_2.sp
bandpass LCR filter, pole/zero
fbpnet.sp
bandpass LCR filter, s-parameters
fbprlc.sp
LCR AC analysis for resonance
fhp4th.sp
high-pass LCR, fourth-order Butterworth filter
fkerwin.sp
pole/zero analysis of Kerwin’s circuit
flp5th.sp
low-pass, fifth-order filter
flp9th.sp
low-pass, ninth-order FNDR, with ideal op-amps
micro1.sp
test of microstrip
micro2.sp
test of microstrip
tcoax.sp
test of RG58/AU coax
HSPICE® Simulation and Analysis User Guide
Y-2006.03
535
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
trans1m.sp
FR-4, printed-circuit, lumped transmission line
Magnetics $installdir/demo/hspice/mag
aircore.sp
air-core transformer circuit
bhloop.sp
b-h loop, non-linear, magnetic-core transformer
mag2.sp
three primary, two secondary, magnetic-core transformer
magcore.sp
magnetic-core transformer circuit
royerosc.sp
Royer magnetic-core oscillator
MOSFET Devices $installdir/demo/hspice/mos
536
bsim3.sp
LEVEL=47 BSIM3 model
cap13.sp
plot MOS capacitances, LEVEL=13 model
cap_b.sp
capacitances for LEVEL=13 model
cap_m.sp
capacitance for LEVEL=13 model
capop0.sp
plot MOS capacitances, LEVEL=2
capop1.sp
plot MOS capacitances, LEVEL=2
capop2.sp
plot MOS capacitances, LEVEL=2
capop4.sp
plot MOS capacitances, LEVEL=6
chrgpump.sp
charge-conservation test, LEVEL=3
iiplot.sp
plot of impact ionization current
ml6fex.sp
plot temperature effects, LEVEL=6
ml13fex.sp
plot temperature effects, LEVEL=13
ml13ft.sp
s-parameters for LEVEL=13
ml13iv.sp
plot I-V for LEVEL=13
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
ml27iv.sp
plot I-V for LEVEL=27 SOSFET
mosiv.sp
plot I-V for files that you include
mosivcv.sp
plot I-V and C-V for LEVEL=3
qpulse.sp
charge-conservation test, LEVEL=6
qswitch.sp
charge-conservation test, LEVEL=6
selector.sp
automatic model selector for width and length
tgam2.sp
LEVEL=6, gamma model
tmos34.sp
MOS LEVEL=34 EPFL, test DC
Radiation Effects $installdir/demo/hspice/rad
brad1.sp
example of bipolar radiation effects
brad2.sp
example of bipolar radiation effects
brad3.sp
example of bipolar radiation effects
brad4.sp
example of bipolar radiation effects
brad5.sp
example of bipolar radiation effects
brad6.sp
example of bipolar radiation effects
drad1.sp
example of diode radiation effects
drad2.sp
example of diode radiation effects
drad4.sp
example of diode radiation effects
drad5.sp
example of diode radiation effects
drad6.sp
example of diode radiation effects
dradarb2.sp
example of diode radiation effects
jex1.sp
example of JFET radiation effects
HSPICE® Simulation and Analysis User Guide
Y-2006.03
537
Chapter 19: Running Demonstration Files
Demonstration Input Files
538
File Name
Description
jex2.sp
example of JFET radiation effects
jprad1.sp
example of JFET radiation effects
jprad2.sp
example of JFET radiation effects
jprad4.sp
example of JFET radiation effects
jrad1.sp
example of JFET radiation effects
jrad2.sp
example of JFET radiation effects
jrad3.sp
example of JFET radiation effects
jrad4.sp
example of JFET radiation effects
jrad5.sp
example of JFET radiation effects
jrad6.sp
example of JFET radiation effects
mrad1.sp
example of MOSFET radiation effects
mrad2.sp
example of MOSFET radiation effects
mrad3.sp
example of MOSFET radiation effects
mrad3p.sp
example of MOSFET radiation effects
mrad3px.sp
example of MOSFET radiation effects
rad1.sp
example of total MOSFET dose
rad2.sp
diode photo-current test circuit
rad3.sp
diode photo-current test circuit, RLEV=3
rad4.sp
diode photo-current test circuit
rad5.sp
BJT photo-current test circuit, with an NPN transistor
rad6.sp
BJT secondary photo-current effect, which varies with R1
rad7.sp
BJT RLEV=6 example (semi-empirical model)
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
rad8.sp
JFET RLEV=1 example with Wirth-Rogers square pulse
rad9.sp
JFET stepwise-increasing radiation source
rad10.sp
GaAs RLEV=5 example (semi-empirical model)
rad11.sp
NMOS E-model, LEVEL=8 with Wirth-Rogers square pulse
rad12.sp
NMOS 0.5x resistive vl(Ru)htage-d-eivGuirse
HSPICE® Simulation and Analysis User Guide
Y-2006.03
539
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
fr4x.sp
FR4 microstrip test
hd.sp
ground bounce for I/O CMOS driver
rcsnubts.sp
ground bounce for I/O CMOS driver, at snubber output
rcsnubtt.sp
ground bounce for I/O CMOS driver
strip1.sp
two microstrips, in series (8 mil and 16 mil wide)
strip2.sp
two microstrips, coupled together
t14p.sp
1400 mil by 140 mil, 50-ohm tline, on FR-4, 50 MHz to 10.05 GHz
t14xx.sp
1400 mil by 140 mil, 50-ohm tline, on FR-4 optimization
t1400.sp
1400 mil by 140 mil, 50-ohm tline, on FR-4 optimization
tcoax.sp
RG58/AU coax, with 50-ohm termination
tfr4.sp
microstrip test
tfr4o.sp
microstrip test
tl.sp
series source, coupled and shunt-terminated transmission lines
transmis.sp
algebraics, and lumped transmission lines
twin2.sp
twin-lead model
xfr4.sp
microstrip test sub-circuit, expanded
xfr4a.sp
microstrip test sub-circuit, expanded, larger ground-resistance
xfr4b.sp
microstrip test
xulump.sp
test 5-, 20-, and 100-lump, U models
Verilog-A $installdir/demo/hspice/veriloga
540
resistor.sp
a very simple Verilog-A resistor model
sinev.sp
simple voltage source
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Chapter 19: Running Demonstration Files
Demonstration Input Files
File Name
Description
deadband.sp
deadband amplifier
pll.sp
behavioral model of PLL
psfet.sp
Parker Skellern FET model
colpitts.va
Colpitts BJT oscillator
ecl.sp
ECL inverter
opamp.sp
opamp
sample_hold.sp sample and hold
biterrorrate.sp
bit error rate counter
dac.sp
DAC and ADC
HSPICE® Simulation and Analysis User Guide
Y-2006.03
541
Chapter 19: Running Demonstration Files
Demonstration Input Files
542
HSPICE® Simulation and Analysis User Guide
Y-2006.03
A
Statistical Analysis
A
Describes the features available in HSPICE for statistical analysis before the
Y-2006.03 release.
Overview
Described in this appendix are the features available in HSPICE for statistical
analysis before the Y-2006.03 release. These features are still supported;
however, the new features described in Chapter 13, Simulating Variability,
Chapter 14, Variation Block, and Chapter 15, Monte Carlo Analysis represent a
significant enhancement over prior approaches.
The previously available documentation on statistical analysis has been
reviewed and enhanced for the benefit of those users who are not yet ready to
migrate to the new approach. In particular, the last section was added to
explain the setup for simulating the effects of global and local variations on
silicon with Monte Carlo.
The following subjects are described in this appendix:
■
Application of Statistical Analysis
■
Analytical Model Types
■
Simulating Circuit and Model Temperatures
■
Worst Case Analysis
■
Monte Carlo Analysis
■
Worst Case and Monte Carlo Sweep Example
■
Simulating the Effects of Global and Local Variations with Monte Carlo
HSPICE® Simulation and Analysis User Guide
Y-2006.03
543
Appendix A: Statistical Analysis
Application of Statistical Analysis
Application of Statistical Analysis
When you design an electrical circuit, it must meet tolerances for the specific
manufacturing process. The electrical yield is the number of parts that meet the
electrical test specifications. Overall process efficiency requires maximum
yield. To analyze and optimize the yield, Synopsys HSPICE supports statistical
techniques and observes the effects of variations in element and model
parameters.
Analytical Model Types
To model parametric and statistical variation in circuit behavior, use:
■
.PARAM statement to investigate the performance of a circuit as you change
circuit parameters. For details about the .PARAM statement, see the
.PARAM statement in the HSPICE Command Reference.
■
Temperature variation analysis to vary the circuit and component
temperatures, and compare the circuit responses. You can study the
temperature-dependent effects of the circuit, in detail.
■
Monte Carlo analysis when you know the statistical standard deviations of
component values to center a design. This provides maximum process
yield, and determines component tolerances.
■
Worst-case corner analysis when you know the component value limit to
automate quality assurance for:
■
544
•
basic circuit function
•
process extremes
•
quick estimation of speed and power trade-offs
•
best-case and worst-case model selection
•
parameter corners
•
library files
Data-driven analysis for cell characterization, response surface, or Taguchi
analysis. See “Performing Digital Cell Characterization” in the HSPICE
Applications Manual. Automates characterization of cells and calculates the
coefficient of polynomial delay for timing simulation. You can simultaneously
vary any number of parameters and perform an unlimited number of
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Simulating Circuit and Model Temperatures
analyses. This analysis uses an ASCII file format so HSPICE can
automatically generate parameter values. This analysis can replace
hundreds or thousands of HSPICE simulation runs.
Use yield analyses to modify:
■
DC operating points
■
DC sweeps
■
AC sweeps
■
Transient analysis.
CosmosScope can generate scatter plots from the operating point analysis or a
family of curve plots for DC, AC, and transient analysis.
Use .MEASURE statements to save results for delay times, power, or any other
characteristic extracted in a .MEASURE statement. HSPICE generates a table
of results in an .mt# file in ASCII format. You can analyze the numbers directly
or read this file into CosmosScope to view the distributions. Also, if you use
.MEASURE statements in a Monte Carlo or data-driven analysis, then the
HSPICE output file includes the following statistical results in the listing:
Mean
Variance
Sigma
x1 + x2 + … + xn
---------------------------------------N
( x 1 – Mean ) 2 + … ( x n – Mean ) 2
------------------------------------------------------------------------------N–1
Variance
Average Deviation
x 1 – Mean + … + x n – Mean
--------------------------------------------------------------------------N–1
Simulating Circuit and Model Temperatures
Temperature affects all electrical circuits. Figure 93 shows the key temperature
parameters associated with circuit simulation:
■
Model reference temperature – you can model different models at different
temperatures. Each model has a TREF (temperature reference) parameter.
■
Element junction temperature – each resistor, transistor, or other element
generates heat so an element is hotter than the ambient temperature.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
545
Appendix A: Statistical Analysis
Simulating Circuit and Model Temperatures
■
Part temperature – at the system level each part has its own temperature.
■
System temperature – a collection of parts form a system, which has a local
temperature.
■
Ambient temperature – the ambient temperature is the air temperature of
the system.
Figure 93
Part Junction Temperature Sets System Performance
Ambient Temperature
System Temperature
source
drain
gate
Model Junction Temperature
Part Temperature
source
drain
gate
Part Junction Temperature
HSPICE or HSPICE RF calculates temperatures as differences from the
ambient temperature:
Tambient + Δsystem + Δpart + Δjunction = Tjunction
Ids = f ( Tjunction, Tmodel )
Every element includes a DTEMP keyword, which defines the difference
between junction and ambient temperature.
Example
The following example uses DTEMP in a MOSFET element statement:
M1 drain gate source bulk Model_name W=10u L=1u DTEMP=+20
546
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Simulating Circuit and Model Temperatures
Temperature Analysis
You can specify three temperatures:
■
Model reference temperature specified in a .MODEL statement. The
temperature parameter is usually TREF, but can be TEMP or TNOM in some
models. This parameter specifies the temperature, in °C, at which HSPICE
or HSPICE RF measures and extracts the model parameters. Set the value
of TNOM in an .OPTION statement. Its default value is 25°C.
■
Circuit temperature that you specify using a .TEMP statement or the TEMP
parameter. This is the temperature, in °C, at which HSPICE or HSPICE RF
simulates all elements. To modify the temperature for a particular element,
use the DTEMP parameter. The default circuit temperature is the value of
TNOM.
■
Individual element temperature, which is the circuit temperature, plus an
optional amount that you specify in the DTEMP parameter.
To specify the temperature of a circuit in a simulation run, use either the .TEMP
statement, or the TEMP parameter in the .DC, .AC, or .TRAN statements.
HSPICE or HSPICE RF compares the circuit simulation temperature that one
of these statements sets against the reference temperature that the TNOM
option sets. TNOM defaults to 25°C, unless you use the SPICE option, which
defaults to 27°C. To calculate the derating of component values and model
parameters, HSPICE or HSPICE RF uses the difference between the circuit
simulation temperature, and the TNOM reference temperature.
Elements and models within a circuit can operate at different temperatures. For
example, a high-speed input/output buffer that switches at 50 MHz is much
hotter than a low-drive NAND gate that switches at 1 MHz). To simulate this
temperature difference, specify both an element temperature parameter
(DTEMP), and a model reference parameter (TREF). If you specify DTEMP in an
element statement, the element temperature for the simulation is:
element temperature=circuit temperature + DTEMP
Specify the DTEMP value in the element statement (resistor, capacitor, inductor,
diode, BJT, JFET, or MOSFET statement), or in a subcircuit element. Assign a
parameter to DTEMP, then use the .DC statement to sweep the parameter. The
DTEMP value defaults to zero.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
547
Appendix A: Statistical Analysis
Worst Case Analysis
If you specify TREF in the model statement, the model reference temperature
changes (TREF overrides TNOM). Derating the model parameters is based on
the difference between circuit simulator temperature and TREF (instead of
TNOM).
.TEMP Statement
To specify the temperature of a circuit for a HSPICE or HSPICE RF simulation,
use the .TEMP statement.
Worst Case Analysis
Circuit designers often use worst-case analysis when designing and analyzing
MOS and BJT IC circuits. To simulate the worst case, set all variables to their 2or 3-sigma worst-case values. Because several independent variables rarely
attain their worst-case values simultaneously, this technique tends to be overly
pessimistic and can lead to over-designing the circuit. However, this analysis is
useful as a fast check.
Model Skew Parameters
The Synopsys HSPICE device models include physically-measurable model
parameters. The circuit simulator uses parameter variations to predict how an
actual circuit responds to extremes in the manufacturing process. Physicallymeasurable model parameters are called skew parameters, because they skew
from a statistical mean to obtain predicted performance variations.
Examples of skew parameters are the difference between the drawn and
physical dimension of metal, postillion, or active layers, on an integrated circuit.
Generally, you specify skew parameters independently of each other, so you
can use combinations of skew parameters to represent worst cases. Typical
skew parameters for CMOS technology include:
548
■
XL – polysilicon CD (critical dimension of the poly layer, representing the
difference between drawn and actual size).
■
XWn, XWp – active CD (critical dimension of the active layer, representing the
difference between drawn and actual size).
■
TOX – thickness of the gate oxide.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case Analysis
■
RSHn, RSHp – resistivity of the active layer.
■
DELVTOn, DELVTOp– variation in threshold voltage.
You can use these parameters in any level of MOS model, within the HSPICE
device models. The DELVTO parameter shifts the threshold value. HSPICE
adds this value to VTO for the Level 3 model, and adds or subtracts it from VFB0
for the BSIM model. Table 60 shows whether HSPICE adds or subtracts
deviations from the average.
Table 60
Sigma Deviations
Type
Parameter
Slow
Fast
NMOS
XL
+
-
RSH
+
-
DELVTO
+
-
TOX
+
-
XW
-
+
XL
+
-
RSH
+
-
DELVTO
-
+
TOX
+
-
XW
-
+
PMOS
HSPICE selects skew parameters based on the available historical data that it
collects either during fabrication or electrical test. For example, HSPICE
collects the XL skew parameter for poly CD during fabrication. This parameter
is usually the most important skew parameter for a MOS process.
Figure 94 is an example of data that historical records produce.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
549
Appendix A: Statistical Analysis
Worst Case Analysis
Figure 94
Historical Records for Skew Parameters in a MOS Process
3 sigma
2 sigma
Fab Database
1 sigma
Run# PolyCD
Mean
101 +0.04u
102 -0.06u
pop.#
103 +0.03u
...
XL value
Using Skew Parameters in HSPICE
Figure 95 on page 550 shows how to create a worst-case corners library file for
a CMOS process model in HSPICE (HSPICE RF does not support worst-case
analysis). Specify the physically-measured parameter variations so that their
proper minimum and maximum values are consistent with measured current
(IDS) variations. For example, HSPICE can generate a 3-sigma variation in IDS
from a 2-sigma variation in physically-measured parameters.
Figure 95
SS
Worst Case Corners Library File for a CMOS Process Model
Slow Corner Skew Parameters
pop.
IDS
The .LIB (library) statement, and the .INCLUDE (include file) statement,
access the models and skew. The library contains parameters that
550
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case Analysis
modify .MODEL statements. The following example of .LIB features both
worst-case and statistical-distribution data by using model skew parameters. In
statistical distribution, the median value is the default for all non-Monte Carlo
analysis (HSPICE RF does not support Monte Carlo analysis).
Example
.LIB TT
$TYPICAL P-CHANNEL AND N-CHANNEL CMOS LIBRARY DATE:3/4/91
$ PROCESS: 1.0U CMOS, FAB22, STATISTICS COLLECTED 3/90-2/91
$ following distributions are 3 sigma ABSOLUTE GAUSSIAN
.PARAM
$ polysilicon Critical Dimensions
+ polycd=agauss(0,0.06u,1) xl=’polycd-sigma*0.06u’
$ Active layer Critical Dimensions
+ nactcd=agauss(0,0.3u,1) xwn=’nactcd+sigma*0.3u’
+ pactcd=agauss(0,0.3u,1) xwp=’pactcd+sigma*0.3u’
$ Gate Oxide Critical Dimensions (200 angstrom +/- 10a at 1
$ sigma)
+ toxcd=agauss(200,10,1) tox=’toxcd-sigma*10’
$ Threshold voltage variation
+ vtoncd=agauss(0,0.05v,1) delvton=’vtoncd-sigma*0.05’
+ vtopcd=agauss(0,0.05v,1) delvtop=’vtopcd+sigma*0.05’
.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=230 XL=-0.18u DELVTON=-.15V DELVTOP= 0.15V
.INC ‘/usr/meta/lib/cmos1_mod.dat’ $ model include file
.ENDL FF
The /usr/meta/lib/cmos1_mod.dat include file contains the model.
.MODEL NCH NMOS LEVEL=2 XL=XL TOX=TOX DELVTO=DELVTON . .
.MODEL PCH PMOS LEVEL=2 XL=XL TOX=TOX DELVTO=DELVTOP . .
Note:
The model keyname (left) equals the skew parameter (right). Model keys
and skew parameters can use the same names.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
551
Appendix A: Statistical Analysis
Worst Case Analysis
Skew File Interface to Device Models
Skew parameters are model parameters for transistor models or passive
components. A typical device model set includes:
■
MOSFET models for all device sizes by using an automatic model selector.
■
RC wire models for polysilicon, metal1, and metal2 layers in the drawn
dimension. Models include temperature coefficients and fringe capacitance.
■
Single-diode and distributed-diode models for N+, P+, and well (includes
temperature, leakage, and capacitance based on the drawn dimension).
■
BJT models for parasitic bipolar transistors. You can also use these for any
special BJTs, such as a BiCMOS for ECL BJT process (includes current and
capacitance as a function of temperature).
■
Metal1 and metal2 transmission line models for long metal lines.
■
Models must accept elements. Sizes are based on a drawn dimension. If
you draw a cell at 2μ dimension and shrink it to 1μ, the physical size is 0.9μ.
The effective electrical size is 0.8μ. Account for the four dimension levels:
•
drawn size
•
shrunken size
•
physical size
•
electrical size
Most simulator models scale directly from drawn to electrical size. HSPICE
MOS models support all four size levels as in Figure 96.
552
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
Figure 96
Device Model from Drawn to Electrical Size
Drawn Size
Shrunken Size
2m
1m
LMLT
WMLT
XL
XW
Electrical Size
source
Physical Size
source
drain
drain
gate
gate
LD
WD
0.8 m
0.9 m
Monte Carlo Analysis
Monte Carlo analysis (HSPICE only; HSPICE RF does not support Monte
Carlo analysis) uses a random number generator to create the following types
of functions.
■
■
■
Gaussian parameter distribution
•
Relative variation—variation is a ratio of the average.
•
Absolute variation—adds variation to the average.
•
Bimodal–multiplies distribution to statistically reduce nominal
parameters.
Uniform parameter distribution
•
Relative variation—variation is a ratio of the average.
•
Absolute variation—adds variation to the average.
•
Bimodal–multiplies distribution to statistically reduce nominal
parameters.
Random limit parameter distribution
•
Absolute variation—adds variation to the average.
•
Monte Carlo analysis randomly selects the min or max variation.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
553
Appendix A: Statistical Analysis
Monte Carlo Analysis
The value of the MONTE analysis keyword determines how many times to
perform operating point, DC sweep, AC sweep, or transient analysis.
Figure 97
Monte Carlo Distribution
Uniform Distribution
Gaussian Distribution
Population
Population
Abs
variation
Abs
variation
3 Sigma
Nom_value
Nom_value
Rel_variation=Abs_variation/Nom_value
Monte Carlo Setup
To set up a Monte Carlo analysis, use the following HSPICE statements:
■
.PARAM statement—sets a model or element parameter to a Gaussian,
Uniform, or Limit function distribution.
■
.DC, .AC, or .TRAN analysis—enables MONTE.
■
.MEASURE statement—calculates the output mean, variance, sigma, and
standard deviation.
■
.MODEL statement—sets model parameters to a Gaussian, Uniform, or
Limit function distribution.
Select the type of analysis to run, such as operating point, DC sweep, AC
sweep, or TRAN sweep.
Operating Point
.DC MONTE=<firstrun=num1>
-or.DC MONTE=list <(> <num1:num2> <num3> <num5:num6> <num7> <)>
554
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
DC Sweep
.DC vin 1 5 0.25 sweep MONTE=val <firstrun=num1>
-or.DC vin 1 5 0.25 sweep MONTE=list<(> <num1:num2> <num3>
+ <num5:num6> <num7> <)>
AC Sweep
.AC dec 10 100 1meg sweep MONTE=val <firstrun=num1>
-or.AC dec 10 100 1meg sweep MONTE=list<(> <num1:num2>
+ <num3> <num5:num6> <num7> <)>
TRAN Sweep
.TRAN 1n 10n sweep MONTE=val <firstrun=num1>
-or.TRAN 1n 10n sweep MONTE=list<(> <num1:num2> <num3>
+ <num5:num6> <num7> <)>
The val value specifies the number of Monte Carlo iterations to perform. A
reasonable number is 30. The statistical significance of 30 iterations is quite
high. If the circuit operates correctly for all 30 iterations, there is a 99%
probability that over 80% of all possible component values operate correctly.
The relative error of a quantity, determined through Monte Carlo analysis, is
proportional to val-1/2.
The firstrun values specify the desired number of iterations. HSPICE runs from
num1 to num1+val-1. The number after firstrun can be a parameter. You can
write only one number after list. The colon represents "from ... to ...". Specifying
only one number makes HSPICE runs only a the one specified point.
Example 1
In this example, HSPICE runs from the 90th to 99th Monte Carlo iterations:
.tran 1n 10 sweep monte=10 firstrun=90
You can write more than one number after list. The colon represents "from ... to
...". Specifying only one number makes HSPICE run only at that single point.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
555
Appendix A: Statistical Analysis
Monte Carlo Analysis
Example 1
In this example, HSPICE begins running at the 10th iteration, then continues
from the 20th to the 30th, at the 40th, and finally from the 46th to 72nd Monte
Carlo iteration. The numbers after list can not be parameter.
.tran 1n 10n sweep monte=list(10 20:30 40 46:72)
Monte Carlo Output
■
.MEASURE statements are the most convenient way to summarize the
results.
■
.PRINT statements generate tabular results, and print the values of all
Monte Carlo parameters.
■
.MCBRIEF determines the output types of the random parameters during
Monte Carlo analysis to improve output performance.
■
If one iteration is out of specification, you can obtain the component values
from the tabular listing. A detailed resimulation of that iteration might help
identify the problem.
■
.GRAPH generates a high-resolution plot for each iteration.
■
By contrast, AvanWaves superimposes all iterations as a single plot so you
can analyze each iteration individually.
.PARAM Distribution Function
This section describes how to use assign a .PARAM parameter in Monte Carlo
analysis. For a general description of the .PARAM statement, see the .PARAM
command in the HSPICE Command Reference.
You can assign a .PARAM parameter to the keywords of elements and models,
and assign a distribution function to each .PARAM parameter. HSPICE
recalculates the distribution function each time that and element or model
keyword uses a parameter. When you use this feature, Monte Carlo analysis
can use a parameterized schematic netlist without additional modifications.
556
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
Syntax
.PARAM xx=UNIF(nominal_val, rel_variation
+ <, multiplier>)
.PARAM xx=AUNIF(nominal_val, abs_variation <,
+ multiplier>)
.PARAM xx=GAUSS(nominal_val, rel_variation, sigma <,
+ multiplier>)
.PARAM xx=AGAUSS(nominal_val, abs_variation, sigma <,
+ multiplier>)
.PARAM xx=LIMIT(nominal_val, abs_variation)
Argument
Description
xx
Distribution function calculates the value of this parameter.
UNIF
Uniform distribution function by using relative variation.
AUNIF
Uniform distribution function by using absolute variation.
GAUSS
Gaussian distribution function by using relative variation.
AGAUSS
Gaussian distribution function by using absolute variation
LIMIT
Random-limit distribution function by using absolute variation.
Adds +/- abs_variation to nominal_val based on whether the
random outcome of a -1 to 1 distribution is greater than or less
than 0.
nominal_val
Nominal value in Monte Carlo analysis and default value in all
other analyses.
abs_variation
AUNIF and AGAUSS vary the nominal_val by +/- abs_variation.
rel_variation
UNIF and GAUSS vary the nominal_val by +/- (nominal_val ⋅
rel_variation).
sigma
Specifies abs_variation or rel_variation at the sigma level. For
example, if sigma=3, then the standard deviation is abs_variation
divided by 3.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
557
Appendix A: Statistical Analysis
Monte Carlo Analysis
Argument
Description
multiplier
If you do not specify a multiplier, the default is 1. HSPICE
recalculates many times and saves the largest deviation. The
resulting parameter value might be greater than or less than
nominal_val. The resulting distribution is bimodal.
Example 1
In this example, each R has an unique variation.
.param mc_var=agauss(0,1,3)
.param val='1000*(1+mc_var)'
v_vin vin 0 dc=1 ac=.1
r1 vin 0 '1000*(1+mc_var)'
r2 vin 0 '1000*(1+mc_var)'
$ +/- 20% swing
Example 2
In this example, each R has an identical variation.
.param mc_var=agauss(0,1,3)
.param val='1+mc_var'
v_vin vin 0 dc=1 ac=.1
r1 vin 0 '1000*val'
r2 vin 0 '1000*val'
$ +/- 20% swing
Example 3
In this example, local variations to an instance parameter are applied by
assigning randomly-generated variations directly to each instance parameter.
Each resistor r1 through r3 receives randomly different resistance values
during each Monte Carlo run.
.param
r1 1 2
r2 3 4
r3 5 6
558
r_local=agauss(...)
r=r_local
r=r_local
r=r_local
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
Example 4
In this example, global variations to an instance parameter are applied by
assigning the variation to an intermediate parameter before assigning it to each
instance parameter. Each resistor r1 through r3 receives the same random
resistance value during each Monte Carlo run.
.param
.param
r1 1 2
r2 3 4
r3 5 6
r_random=agauss(...)
r_global=r_random
r=r_global
r=r_global
r=r_global
Monte Carlo Parameter Distribution
Each time you use a parameter, Monte Carlo calculates a new random variable.
■
If you do not specify a Monte Carlo distribution, then HSPICE assumes the
nominal value.
■
If you specify a Monte Carlo distribution for only one analysis, HSPICE uses
the nominal value for all other analyses.
You can assign a Monte Carlo distribution to all elements that share a common
model. The actual element value varies according to the element distribution. If
you assign a Monte Carlo distribution to a model keyword, then all elements
that share the model, use the same keyword value. You can use this feature to
create double element and model distributions.
For example, the MOSFET channel length varies from transistor to transistor by
a small amount that corresponds to the die distribution. The die distribution is
responsible for offset voltages in operational amplifiers, and for the tendency of
flip-flops to settle into random states. However, all transistors on a die site vary
according to the wafer or fabrication run distribution. This value is much larger
than the die distribution, but affects all transistors the same way. You can
specify the wafer distribution in the MOSFET model to set the speed and power
dissipation characteristics.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
559
Appendix A: Statistical Analysis
Monte Carlo Analysis
Monte Carlo Examples
Note:
HSPICE supports Monte Carlo analysis; HSPICE RF does not.
Gaussian, Uniform, and Limit Functions
This example is based on demonstration netlist mont1.sp, which is available in
directory $<installdir>/demo/hspice/apps:
mont1.sp test of monte carlo gaussian, uniform, and limit functions
.option post
.dc monte=60
* setup plots
.probe
.probe
.probe
.probe
.probe
aunif_1=v(au1)
aunif_10=v(au10)
agauss_1=v(ag1)
agauss_10=v(ag10)
limit=v(l1)
* uniform distribution relative variation +/- .2
.param ru_1=unif(100,.2)
iu1 u1 0 -1
ru1 u1 0 ru_1
* absolute uniform distribution absolute variation +/- 20
* single throw and 10 throw maximum
.param rau_1=aunif(100,20)
.param rau_10=aunif(100,20,10)
iau1 au1 0 -1
rau1 au1 0 rau_1
iau10 au10 0 -1
rau10 au10 0 rau_10
* gaussian distribution relative variation +/- .2 at 3 sigma
.param rg_1=gauss(100,.2,3)
ig1 g1 0 -1
rg1 g1 0 rg_1
560
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
* absolute gaussian distribution absolute variation +/- .2 at 3
sigma
* single throw and 10 throw maximum
.param rag_1=agauss(100,20,3)
.param rag_10=agauss(100,20,3,10)
iag1 ag1 0 -1
rag1 ag1 0 rag_1
iag10 ag10 0 -1
rag10 ag10 0 rag_10
* random limit distribution absolute variation +/- 20
.param rl=limit(100,20)
il1 l1 0 -1
rl1 l1 0 rl
.end
Figure 98
119.182
Uniform Functions
MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS
May 15 2003 11:41:23
MONT1_SV0
RUNIF_1
110.0
VOLT [LIN]
100.0
90.0
80.1384
120.0
MONT1_SV0
RUNIF_10
110.0
100.0
90.0
80.0402
1.0
10.0
20.0
30.0
40.0
50.0
60.0
MONTE CARLO [LIN]
HSPICE® Simulation and Analysis User Guide
Y-2006.03
561
Appendix A: Statistical Analysis
Monte Carlo Analysis
Figure 99
115.0
Gaussian Functions
MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS
May 15 2003 11:41:23
MONT1_SV
RGAUSS_1
110.0
VOLT [LIN]
105.0
100.0
95.0
90.0
MONT1_SV
RGAUSS_1
118.375
110.0
100.0
90.0
80.9998
1.0
10.0
20.0
30.0
40.0
50.0
60.0
MONTE CARLO [LIN]
562
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
Figure 100 Limit Functions
MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS
May 15 2003 11:41:23
MONT1.SV0
LIMIT
120.0
115.0
110.0
VOLT [LIN]
105.0
100.0
95.0
90.0
85.0
80.0
1.0
10.0
20.0
30.0
40.0
50.0
60.0
MONTE CARLO [LIN]
Major and Minor Distribution
In MOS IC processes, manufacturing tolerance parameters have both a major
and a minor statistical distribution.
■
The major distribution is the wafer-to-wafer and run-to-run variation. It
determines electrical yield.
■
The minor distribution is the transistor-to-transistor process variation. It is
responsible for critical second-order effects, such as amplifier offset voltage
and flip-flop preference.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
563
Appendix A: Statistical Analysis
Monte Carlo Analysis
Figure 101 Major and Minor Distribution of Manufacturing Variations
major distribution
minor distribution
pop.#
XL
(polysilicon linewidth variation)
The following example is a Monte Carlo analysis of a DC sweep in HSPICE.
(Note that HSPICE supports Monte Carlo analysis; HSPICE RF does not.)
Monte Carlo sweeps the VDD supply voltage from 4.5 volts to 5.5 volts.
This example is based on demonstration netlist mondc_a.sp, which is available
in directory $<installdir>/demo/hspice/apps:
■
The M1 through M4 transistors form two inverters.
■
The nominal value of the LENGTH parameter sets the channel lengths for the
MOSFETs, which are set to 1u in this example.
■
All transistors are on the same integrated circuit die. The LEFF parameter
specifies the distribution—for example, a ±5% distribution in channel length
variation at the ±3-sigma level.
■
Each MOSFET has an independent random Gaussian value.
file: mondc_a.sp
.options post
.dc vdd 4.5 5.5 .1 sweep monte=30
.probe dc i(m1)
vdd 3 0 5v
.param length=1u lphoto=.1u
.param leff=gauss(length,.05,3) xphoto=gauss(lphoto,.3,3)
.param photo=xphoto
m1 1 2 gnd gnd nch w=10u l=leff
m2 1 2 vdd vdd pch w=20u l=leff
m3 2 3 gnd gnd nch w=10u l=leff
m4 2 3 vdd vdd pch w=20u l=leff
.model nch nmos level=2 uo=500 tox=100 gamma=.7 vto=.8 xl=photo
.model pch pmos level=2 uo=250 tox=100 gamma=.5 vto=-.8 xl=photo
.end
The PHOTO parameter controls the difference between the physical gate length
and the drawn gate length. Because both n-channel and p-channel transistors
564
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
use the same layer for the gates, Monte Carlo analysis sets XPHOTO
distribution to the PHOTO local parameter.
XPHOTO controls PHOTO lithography for both NMOS and PMOS devices, which
is consistent with the physics of manufacturing.
RC Time Constant
This simple example shows uniform distribution for resistance and capacitance.
It also shows the resulting transient waveforms for 10 different random values.
This example is based on demonstration netlist rc_monte.sp, which is available
in directory $<installdir>/demo/hspice/apps:
*FILE: MON1.SP WITH UNIFORM DISTRIBUTION
.OPTION LIST POST
.PARAM RX=UNIF(1, .25) CX=UNIF(1, .25)
.TRAN .1 1 SWEEP MONTE=10
.IC 1 1
R1 1 0 RX
C1 1 0 CX
.PRINT I(R1) I(C1)
.END
HSPICE® Simulation and Analysis User Guide
Y-2006.03
565
Appendix A: Statistical Analysis
Monte Carlo Analysis
Figure 102 Monte Carlo Analysis of RC Time Constant
*FILE: NOM1.SP WITH UNIFORM DISTRIBUTION
May 15 2003 12:38:49
MONT1.SV0
1
992.750N
900.0N
VOLT [LIN]
800.0N
700.0N
600.0N
10
500.0N
9
8
400.0N
7
5
26
3
1
300.0N
0
200.0N
400.0N
600.0N
800.0N
1.0
TIME [LIN]
Switched Capacitor Filter Design
Capacitors used in switched-capacitor filters consist of parallel connections of a
basic cell. Use Monte Carlo techniques in HSPICE to estimate the variation in
total capacitance. The capacitance calculation uses two distributions:
566
■
Minor (element) distribution of cell capacitance from cell-to-cell on a single
die.
■
Major (model) distribution of the capacitance from wafer-to-wafer or from
manufacturing run-to-run.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Monte Carlo Analysis
Figure 103 Monte Carlo Distribution
cap-to-cap
(element)
C1a
C1b
C1a
C1b
C1c
C1d
C1c
C1d
run-to-run
(model)
You can approach this problem from physical or electrical levels.
■
The physical level relies on physical distributions, such as oxide thickness
and polysilicon line width control.
■
The electrical level relies on actual capacitor measurements.
Physical Approach:
1. Since oxide thickness control is excellent for small areas on a single wafer,
you can use a local variation in polysilicon to control the variation in
capacitance for adjacent cells.
2. Next, define a local poly line-width variation and a global (model-level) poly
line-width variation. In this example:
•
The local polysilicon line width control for a line 10 m wide,
manufactured with process A, is ±0.02 m for a 1-sigma distribution.
•
The global (model level) polysilicon line-width control is much wider; use
0.1 m for this example.
3. The global oxide thickness is 200 angstroms with a ±5 angstrom variation at
1 sigma.
4. The cap element is square with local poly variation in both directions.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
567
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
5. The cap model has two distributions:
•
poly line-width distribution
•
oxide thickness distribution.
The effective length is:
Leff=Ldrawn - 2 ⋅ DEL
The model poly distribution is half the physical per-side values:
C1a 1 0 CMOD W=ELPOLY L=ELPOLY
C1b 1 0 CMOD W=ELPOLY L=ELPOLY
C1C 1 0 CMOD W=ELPOLY L=ELPOLY
C1D 1 0 CMOD W=ELPOLY L=ELPOLY
$ 10U POLYWIDTH,0.05U=1SIGMA
$ CAP MODEL USES 2*MODPOLY .05u= 1 sigma
$ 5angstrom oxide thickness AT 1SIGMA
.PARAM ELPOLY=AGAUSS(10U,0.02U,1)
+ MODPOLY=AGAUSS(0,.05U,1)
+ POLYCAP=AGAUSS(200e-10,5e-10,1)
.MODEL CMOD C THICK=POLYCAP DEL=MODPOLY
Electrical Approach:
The electrical approach assumes no physical interpretation, but requires a local
(element) distribution and a global (model) distribution. In this example:
■
You can match the capacitors to ±1% for the 2-sigma population.
■
The process can maintain a ±10% variation from run to run for a 2-sigma
distribution.
C1a 1 0 CMOD SCALE=ELCAP
C1b 1 0 CMOD SCALE=ELCAP
C1C 1 0 CMOD SCALE=ELCAP
C1D 1 0 CMOD SCALE=ELCAP
.PARAM ELCAP=Gauss(1,.01,2) $ 1% at 2 sigma
+ MODCAP=Gauss(.25p,.1,2) $10% at 2 sigma
.MODEL CMOD C CAP=MODCAP
Worst Case and Monte Carlo Sweep Example
The following example measures the delay and the power consumption of two
inverters. Additional inverters buffer the input and load the output.
This netlist contains commands for two sets of transient analysis: parameter
sweep from -3 to +3-sigma, and a Monte Carlo analysis. It creates one set of
568
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
output files (mt0 and tr0) for the sigma sweep, and one set (mt1 and tr1) for
Monte Carlo.
$ inv.sp sweep mosfet -3 sigma to +3 sigma, use measure output
.param vref=2.5 sigma=0
.global 1
vcc 1 0 5.0
vin in 0 pwl 0,0 0.2n,5
x1 in 2 inv
x2 2 3 inv
x3 3 out inv
x4 out 4 inv
.macro inv in out
mn out in 0 0 nch w=10u l=1u
mp out in 1 1 pch w=10u l=1u
.eom
.param mult1=1
+ polycd=agauss(0,0.06u,1)
xl='polycd-sigma*0.06u'
+ nactcd=agauss(0,0.3u,1) xwn='nactcd+sigma*0.3u'
+ pactcd=agauss(0,0.3u,1) xwp='pactcd+sigma*0.3u'
+ toxcd=agauss(200,10,1)
tox='toxcd-sigma*10'
+ vtoncd=agauss(0,0.05v,1) delvton='vtoncd-sigma*0.05'
+ vtopcd=agauss(0,0.05v,1) delvtop='vtoncd+sigma*0.05'
+ rshncd=agauss(50,8,1)
rshn='rshncd-sigma*8'
+ rshpcd=agauss(150,20,1)
rshp='rshpcd-sigma*20'
* level=28 example model
.model nch nmos
+ level=28 lmlt=mult1 wmlt=mult1 wref=22u lref=4.4u
+ xl=xl xw=xwn tox=tox delvto=delvton rsh=rshn
...
.model pch pmos
+ level=28 lmlt=mult1 wmlt=mult1 wref=22u lref=4.4u
+ xl=xl xw=xwp tox=tox delvto=delvtop rsh=rshp
+ ld=0.08u wd=0.2u acm=2 ldif=0 hdif=2.5u
+ rs=0 rd=0 rdc=0 rsc=0 rsh=rshp js=3e-04 jsw=9e-10
...
* transient with sweep
.tran 20p 1.0n
sweep sigma -3 3 .5
.meas s_delay trig v(2) val=vref fall=1
+
targ v(out) val=vref fall=1
.meas s_power rms power
* transient with Monte Carlo
.tran 20p 1.0n
sweep monte=100
.meas m_delay trig v(2) val=vref fall=1
+
targ v(out) val=vref fall=1
.meas m_power rms power
.probe tran v(in) v(1) v(2) v(3) v(4)
.end
HSPICE® Simulation and Analysis User Guide
Y-2006.03
569
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Transient Sigma Sweep Results
The plot in Figure 104 shows the family of transient analysis curves for the
transient sweep of the sigma parameter from -3 to +3 from the file inv.tr0. In the
sweep, HSPICE uses the values of sigma to update the skew parameters,
which in turn modify the actual NMOS and PMOS models.
Figure 104 Sweep of Skew Parameters from -3 Sigma to +3 Sigma
To view the measured results, plot the inv.mt0 output file. The plot in Figure 105
shows the measured pair delay and the total dissipative power, as a function of
the parameter sigma.
570
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Figure 105 Sweep MOS Inverter, Pair Delay and Power: -3 Sigma to 3 Sigma
Monte Carlo Results
This section describes the output of the Monte Carlo analysis in HSPICE. The
plot in Figure 106 shows that the relationship between TOX against XL
(polysilicon width=transistor length)) is completely random, as set up in the
input file.
To generate this plot in CosmosScope:
1. Read in the file inv.mt1.
2. Open the Calculator, select TOX (left mouse button), transfer to calculator
(middle mouse button), and then select and transfer XL.
3. On the WAVE pulldown in the calculator, select f(x), and then click the plot
icon.
4. Using the right mouse button on the plotted waveform, select Attributes to
change from the line plot to symbols.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
571
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Figure 106 Scatter Plot, XL and TOX
The next graph (see Figure 107) is a standard scatter plot showing the
measured delay for the inverter pair against the Monte Carlo index number.
572
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Figure 107 Scatter Plot of Inverter Pair Delay
If a particular result looks interesting; for example, if the simulation 68 (monte
carlo index=68) produces the smallest delay, then you can obtain the Monte
Carlo parameters for that simulation.
*** monte carlo index =
68 ***
MONTE CARLO PARAMETER DEFINITIONS
polycd xl
= -1.6245E-07
nactcd xwn
= 3.4997E-08
pactcd xwp
= 3.6255E-08
toxcd
tox
=
191.0
vtoncd delvton
= -2.2821E-02
delvtop
= 4.1776E-02
vtopcd
rshncd rshn
=
45.16
rshpcd rshp
=
166.2
m_delay= 1.7929E-10 targ= 3.4539E-10
m_power= 6.6384E-03 from= 0.0000E+00
trig=
to=
1.6610E-10
1.0000E-09
In the preceding listing, the m_delay value of 1.79e-10 seconds is the fastest
pair delay. You can also examine the Monte Carlo parameters that produced
this result.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
573
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
The information on shortest delay and so forth is also available from the
statistics section at the end of the output listing. While this information is useful
to determine whether the circuit meets specification, it is often desirable to
understand the relationship of the parameters to circuit performance. Plotting
the results against the Monte Carlo index number does not help for this
purpose. You need to generate plots that display a Monte Carlo result as a
function of a parameter. For example, Figure 108 shows the inverter pair delay
to channel as a function of poly width, which relates directly to device length.
Figure 108 Delay as a function of Poly width (XL)
Figure 109 shows the pair delay against the TOX parameter. The scatter plot
shows no obvious dependence, which means that the effect of TOX is much
smaller than XL. To explore this in more detail, set the XL skew parameter to a
constant and run a simulation.
574
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Figure 109 Sensitivity of Delay with TOX
The plot in Figure 110 overlays the skew result with the ones from Monte Carlo.
The skew simulation traverses the design space with all parameters changing
in parallel and then produces a relationship between power and delay, which
shows as a single line. Monte Carlo exercises a variety of independent
parameter combinations, and shows that there is no simple relationship
between the two results. Since the distributions were defined as Gaussian in
the netlist, parameter values close to the nominal are more often exercised
than the ones far away. With the relatively small number of samples, the chance
of hitting a combination at the extremes is very small. In other words, designing
for 3-sigma extreme for every parameter is probably not a good solution from
the point of view of economy.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
575
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Figure 110 Superimposing Sigma Sweep Over Monte Carlo
Figure 111 superimposes the required part grades for product sales onto the
Monte Carlo plot. This example uses a 250 ps delay and 6.0 mW power
dissipation to determine the four binning grades.
576
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Worst Case and Monte Carlo Sweep Example
Figure 111 Speed/Power Yield Estimation
Sorting the results from inv.mt1 yields:
■
Bin1 - 18%
■
Bin2 - 30%
■
Bin3 - 31%
■
Bin4 - 21%
If this circuit is representative of the entire chip, then the present yield should
be 18% for the premium Bin 1 parts, assuming variations in process
parameters as specified in the netlist. Of course this example only shows the
principle on how to analyze the Monte Carlo results; there is no market for a
device with two of these inverters.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
577
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
Simulating the Effects of Global and Local Variations with Monte Carlo
Monte Carlo analysis is dependent on a method to describe variability. Four
different approaches are available in HSPICE:
■
specify distributions on parameters and apply these to instance parameters
■
specify distributions on parameters and apply these to model parameters
■
specify distributions on model parameters using DEV/LOT construct
■
specify distributions on model parameters in a variation block.
While the first three methods are still supported in HSPICE, the method based
on the variation block emphasized here for improvements and future
developments. The variation block is described in Chapter 14, Variation Block,
and Monte Carlo analysis controlled by the variation block is described in
Chapter 15, Monte Carlo Analysis.
In the following sections, the first three methods are described. The description
relies on test cases, which can be found in the tar file monte_test.tar in
directory $<installdir>/demo/hspice/apps.
Variations Specified on Geometrical Instance Parameters
This method consists of defining parameters with variation using the
distribution functions UNIF, AUINF, GAUSS, AGAUSS, and LIMIT. These
parameters are then used to generate dependent parameters or in the place of
instance parameters. In a Monte Carlo simulation, at the beginning of each
sample, new random values are calculated for these parameters. For each
reference, a new random value is generated; however, no new value is
generated for a derived parameter. Therefore, it is possible to apply
independent variations to parameters of different devices, as well as the same
variation to parameters of a group of devices. Parameters that describe
distributions can be used in expressions, thus it is possible to create
combinations of variations (correlations).
These concepts are best explained with circuit examples. In the three following
examples, variation is defined on the width of a physical resistor, which has a
model. If this device was a polysilicon resistor for example, then the variations
describe essentially the effects of photoresist exposure and etching on the
width of the poly layer.
578
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
■
test1.sp has a distribution parameter defined called globw. A parameter
called globwidth is assigned the value of globw. The parameter globwidth is
assigned a different random value for each Monte Carlo sample. The
parameter globwidth is used to define the width of the physical resistors r1,
r2, r3, and r4, with model “resistor”. Since parameter globwidth does not
have its own distribution defined, but rather gets its value from the parameter
globw, the value for globwidth is the same wherever it is used; thus the
resistors have the same width for each Monte Carlo sample, and therefore
the same resistance. When plotting the simulation results v1, v2, v3, and v4
from the .meas file, the waveforms overlay perfectly. This type of setup is
typically used to model global variations, which means variations that affect
all devices the same way.
■
test2.sp has a distribution parameter defined called locwidth. This
parameter is used to define the width of the physical resistors r1, r2, r3, and
r4, with model “resistor”. Since the parameter has its own distribution
defined, its value will be different for each reference, and of course for each
Monte Carlo sample. Therefore, the resistors will always have different
values, and the voltages will be different. This type of setup is typically used
to model local variations, which means variations that affect devices in a
different way.
■
test3.sp has two kinds of distributions defined: globw/globwidth as in the first
example, and locwidth as in the second example. The sum of the two is used
to define the width of the resistors. Therefore, the resistors will always have
different widths: a common variation due to globwidth and a separate
variation due to locwidth. In the example, the distribution for locwidth was
chosen as narrower than for globwidth. When overlaying the measurement
results, the large common variation can easily be seen; however, all
voltages are different.
In summary, each reference to a parameter with a specified distribution causes
a new random variable to be generated for each Monte Carlo sample. When
referencing the parameter on an instance, the effect of a local variation is
created. When referencing the parameter on an expression for a second
parameter and using the second parameter on an instance, then the effect of a
global variation is created.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
579
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
Variations Specified in the Context of Subcircuits
The concept explained in the previous section applies also to subcircuits as
instances, and instances within subcircuits. Here we again use the example of
a physical resistor, with variation of its width.
580
■
test4.sp uses a subcircuit for each resistor instead of the top-level resistors
in test3.sp. On each subcircuit, a parameter “width” is assigned a value by
an expression, which is the same for all of them. This value is then passed
into the subcircuit and the resistor width gets this value. Because the
expression is the same for all subcircuits, the value of parameter “width” will
be the same for all subcircuits, thus it expresses a global variation.
Therefore all resistors have the same width, and the terminal voltages are
the same.
■
In test5.sp, if a different “width” is used for the subcircuits, then the
expressions are treated separately, get local variation assigned, and
different values are passed into the subcircuit. In test5.sp, the differences
inside of the expressions are kept numerically very small, thus the
differences from the different values of “locwidth” are dominant and the
results look almost identical to the ones from test3.sp.
■
In test6.sp, the resistor width is assigned inside of the subcircuit. The
variations get picked up from the top level. Because each subcircuit is a
separate entity, the parameter “w” is treated as a separate reference, thus
each resistor will have its own value, partly def
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
In summary, each subcircuit has its own parameter space, therefore it is
possible to put groups of identical components into a subcircuit, and within
each group all devices have the same parameter values, but between the
groups, parameters are different. When specifying variations on these
parameters, the effects of local variations between the groups are created.
Variations on a Model Parameter Using a Local Model in
Subcircuit
If a model is specified within a subcircuit, then the specified parameter values
apply only to the devices in the same subcircuit. Therefore, it is possible to
calculate the value of a model parameter within the subcircuit; for example, as
a function of geometry information.
When specifying variations on these parameters, the effects of local variations
between subcircuits are created. If this method is used at the extreme with one
device per subcircuit, then each device has its own model. This approach leads
to a substantial overhead in the simulator and is therefore not recommended.
Indirect Variations on a Model Parameter
In sections Variations Specified on Geometrical Instance Parameters and
Variations Specified in the Context of Subcircuits, variations on geometrical
parameters were presented. If we want to specify variations on a model
parameter; for example, the threshold of a MOS device, then the approach
explained in the previous section with one model per device in a subcircuit
could be used. However, this is impractical because the netlist needs to be
created to call each device as a subcircuit, and because of the overhead. Since
variations are of interest only on a few model parameters, an indirect method of
varying model parameters can be used. Some special instance parameters are
available for this purpose. For example, for MOS devices, the parameter delvt0
defines a shift in threshold.
Referencing a parameter with a distribution as value for delvt0 creates the
effect of local threshold variations. A significant number of parameters of this
type are available in HSPICE for BSIM3 and BSIM4 models. The variations can
be tailored for each device depending on its size for example. A disadvantage
of this method is that the netlist needs to be parameterized properly to get the
correct variations. The process of preparing a basic netlist for Monte Carlo
simulations with this approach is tedious and error prone, therefore it is best
handled with scripts.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
581
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
Bsim3 supports the following instance parameters:
L, w, ad, as, pd, ps, nrd, nrs, rdc, rsc, off, ic, dtemp, delvto, geo, sa, sb, sd, nf,
stimod, sa1, sa2, sa3, sa4, sa5, sa6, sa7, sa8, sa9, sa10, sb1, sb2, sb3, sb4,
sb5, sb6, sb7, sb8, sb9, sb10, sw1, sw2, sw3, sw4, sw5, sw6, sw7, sw8, sw9,
sw10, mulu0, mulua, mulub, tnodeout, rth0, cth0, deltox, delk1, delnfct, and
acnqsmod.
Bsim4 supports the following instance parameters:
L, w, ad, as, pd, ps, nrd, nrs, rdc, rsc, off, ic, dtemp, delvto, geo, rbsb, rbdb,
rbpb, rbps, rbpd, trnqsmod, acnqsmod, rbodymod, rgatemod, geomod,
rgeomod, nf, min, mulu0, delk1, delnfct, deltox, sa, sb, sd, stimod, sa1, sa2,
sa3, sa4, sa5, sa6, sa7, sa8, sa9, sa10, sb1, sb2, sb3, sb4, sb5, sb6, sb7, sb8,
sb9, sb10, sw1, sw2, sw3, sw4, sw5, sw6, sw7, sw8, sw9, sw10, xgw, ngcon,
sca, scb, scc, sc, delk2, delxj, mulngate, delrsh, delrshg, dellpe0, deldvt0, and
mulvsat.
Variations Specified on Model Parameters
In this section, we investigate the method of specifying distributions on
parameters and using these parameters to define values of model parameters.
With this approach, the netlist does not have to be parameterized. The
modmonte option can be used to distinguish between global variations (all
devices of a particular model have the same parameter set) or local variations
(every device has a unique random value for the specified parameters).
■
test10.sp shows a simple case where the model parameter for sheet
resistivity is assigned a distribution defined on the parameter rsheet. The
results show that all resistors have the same value for each Monte Carlo
sample, but a different one for different samples. This setup is useful for
studying global variations.
■
test11.sp has .option modmonte=1 added. Now every resistor has a
different value.
Note that .option modmonte has no effect on any other approach presented
here.
In summary, assigning parameters with specified distributions to model
parameters allows for investigating the effects of global or local variations, but
not both. The possibility of selecting one or the other with a simple option is
misleading in the sense that the underlying definitions for global and local
variations are not the same for a realistic semiconductor technology.
582
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
Variations Specified Using DEV and LOT
The two limitations of the approach described in section Variations Specified on
Model Parameters are resolved in this method by specifying global and local
variations directly on a model parameter with the syntax:
parameterName=parameterValue LOT/distribution LotDist
+ DEV/distribution DevDist
Where,
LOT keyword for global distribution
DEV keyword for local distribution
distribution is as explained in section Variations Specified on Geometrical
Instance Parameters
LotDist, DevDist characteristic number for the distribution. 3-sigma
value for Gaussian distributions.
■
test12.sp has large global and small local variation, similar to the setup in
the file test3.sp The result shows four different curves, with a large common
part and small separate parts. The amount of variation defined in the two
files is the same. The curves look different from the test3.sp results,
because different random sequences are used. However the statistical
results (sigma) converge for a large number of samples.
There is no option available to select only local or only global variations. This
can be an obstacle if the file is read-only or encrypted.
Combinations of Variation Specifications
Specifying distributions on parameters and applying them to model parameters
can be used on some models and the DEV/LOT approach on others in the same
simulation.
■
test13.sp has DEV/LOT specified for model res1, and the parameter “width”
for model res2. The values for the resistors with model res1 are different,
and the values for resistors with model res2 are the same.
■
test14.sp is similar to test7.sp and has modmonte=1 specified. All four
resistors have different values. However, note that in reality, the sigma for
width would be different when simulating local or global variations.
■
test15.sp has instance parameter variations specified on two resistors and
DEV/LOT on two others. From the waveforms, v3 and v4 form a first pair, and
v1 and v2 a second pair.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
583
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
It is also possible to mix variations on instance parameters and model
parameters in the same setup.
■
test16.sp has small instance parameter variations specified on width and
relatively large model parameter variations on the sheet resistivity, rsh. The
results show four different waveforms, with a common behavior.
■
test17.sp shows instance and model parameter variations as in the previous
test case, but .option modmonte is set to 1, thus the model variations
affect every device in a different way. The results show completely
independent behavior of all four resistors.
If an instance parameter or instance parameter variations and model parameter
variations are specified on the same parameter, then the instance parameter
always overrides the model parameter. Because only few parameters can be
used in both domains, this case is rather seldom, but it needs to be considered
to avoid unexpected results.
■
test18.sp has model variation specified on width with a parameter. Two
resistors have width also defined on instance. The resistors with instance
parameter do not vary at all. The other two resistors vary independently, as
expected because .option modmonte is set to 1.
■
test19.sp is similar to test18.sp with .option modmonte set to 0. The two
resistors that do not have width defined on the instance line vary together.
■
test20.sp has DEV/LOT specified. Instance parameters override variations
on selected resistors.
Variation on Model Parameters as a Function of Device
Geometry
For local variations (see DC Mismatch Analysis), it is a common requirement to
specify variation on a model parameter as a function of device geometry. For
example, the MOS device threshold was observed to vary with the total device
area.
The approach explained in the section Indirect Variations on a Model
Parameter can be used. While this allows for specifying local variations on each
device, it does not include the capability of using expressions based on
element parameters. Thus, variation cannot be described with an expression
that includes the device’s geometry. Conceptually, a netlist processor could be
written that inserts the appropriate values for the parameters as a function of
device size. (Synopsys does not make such a tool available).
584
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
The DEV/LOT approach has no mechanism to describe variation as a function
of an element parameter.
Conclusion
The three approaches described above for specifying variations are not well
suited for semiconductor technologies, because of one or more of the following
issues:
■
require changes to netlist
■
difficult to recognize whether a variation is global or local
■
no way to describe variability as a function of device size
■
no way to run only global or only local variation.
To overcome these issues, a new approach was introduced in HSPICE. This
approach is based on a so called variation block. See chapter 14 For details on
the variation block, see Chapter 14, Variation Block, and for details on how
Monte Carlo analysis is processed with this new approach, see Chapter 15,
Monte Carlo Analysis.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
585
Appendix A: Statistical Analysis
Simulating the Effects of Global and Local Variations with Monte Carlo
586
HSPICE® Simulation and Analysis User Guide
Y-2006.03
B
Full Simulation Examples
B
Contains information and sample input netlists for two full simulation examples.
The examples in this chapter show the basic text and post-processor output for
two sample input netlists.
Note:
The examples are for Synopsys HSPICE, but with minimal modifications,
you can also apply these examples to HSPICE RF.
The first example uses AvanWaves to view results. The second example uses
CosmosScope.
Simulation Example Using AvanWaves
Input Netlist and Circuit
This example is based on demonstration netlist example.sp, which is available
in directory $<installdir>/demo/hspice/bench. This example is an input netlist
for a linear CMOS amplifier. Comment lines indicate the individual sections of
the netlist.
* Example HSPICE netlist, using a linear CMOS amplifier
* netlist options
.option post probe brief nomod
* defined parameters
.param analog_voltage=1.0
* global definitions
.global vdd
* source statements
Vinput in gnd SIN ( 0.0v analog_voltage 10x )
Vsupply vdd gnd DC=5.0v
* circuit statements
HSPICE® Simulation and Analysis User Guide
Y-2006.03
587
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Rinterm in gnd 51
Cincap in infilt 0.001
Rdamp infilt clamp 100
Dlow gnd clamp diode_mod
Dhigh clamp vdd diode_mod
Xinv1 clamp inv1out inverter
Rpull clamp inv1out 1x
Xinv2 inv1out inv2out inverter
Routterm inv2out gnd 100x
* subcircuit definitions
.subckt inverter in out
Mpmos out in vdd vdd pmos_mod l=1u w=6u
Mnmos out in gnd gnd nmos_mod l=1u w=2u
.ends
* model definitions
.model pmos_mod pmos level=3
.model nmos_mod nmos level=3
.model diode_mod d
* analysis specifications
.TRAN 10n 1u sweep analog_voltage lin 5 1.0 5.0
* output specifications
.probe TRAN v(in) v(clamp) v(inv1out) v(inv2out) i(dlow)
.measure TRAN falltime TRIG v(inv2out) VAL=4.5v FALL=1
+ TARG V(inv2out) VAL=0.5v FALL=1
.end
Figure 112 on page 589 is a circuit diagram for the linear CMOS amplifier in the
circuit portion of the netlist. The two sources in the diagram are also in the
netlist.
Note:
The inverter symbols in the circuit diagram are constructed from two
complementary MOSFET elements. Also, the diode and MOSFET models
in the netlist do not have non-default parameter values, except to specify
Level 3 MOSFET models (empirical model).
588
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Figure 112 Circuit Diagram for Linear CMOS Inverter
+5V
Analog
Source
10 MHz
1V to 5V
10 MOhm
0.001 F
100 Ohm
Output
Node
100 MOhm
51 Ohm
Execution and Output Files
The following section displays the output files from a HSPICE simulation of the
amplifier shown in the previous section. To execute the simulation, enter:
hspice example.sp > example.lis
In this syntax, the input netlist name is example.sp, and the output listing file
name is example.lis. Simulation creates the following output files:
Table 61
HSPICE Output Files
Filename
Description
example.ic
Initial conditions for the circuit.
example.lis
Text simulation output listing.
example.mt0
Post-processor output for .MEASURE statements.
example.pa0
Subcircuit path table.
example.st0
Run-time statistics.
example.tr0
Post-processor output for transient analysis.
The following subsections show text files to simulate the amplifier by using
HSPICE on a Sun workstation. The example does not show the two postprocessor output files, which are in binary format.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
589
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Example.ic
* "simulator" "HSPICE"
* "version" "98.4 (981215) "
* "format" "HSP"
* "rundate" "13:58:43 01/08/1999"
* "netlist" "example.sp "
* "runtitle" "* example hspice netlist using a linear
* cmos amplifier "
* time= 0.
* temperature= 25.0000
*** BEGIN: Saved Operating Point ***
.option gmindc= 1.0000p
.nodeset
+ clamp= 2.6200
+ in= 0.
+ infilt= 2.6200
+ inv1out= 2.6200
+ inv2out= 2.6199
+ vdd= 5.0000
***
END: Saved Operating Point ***
Example.lis
Using: /net/sleepy/l0/group/hspice/98.4beta/sol4/hspice
****** HSPICE -- 98.4 (981215) 13:58:43 01/08/1999 solaris
Copyright (C) 1985-2002 by Synopsys Corporation.
Unpublished-rights reserved under US copyright laws.
This program is protected by law and is subject to the
terms and conditions of the license agreement found in:
/afs/rtp.synopsys.com/product/hspice/current/license.txt
Use of this program is your acceptance to be bound by this
license agreement. HSPICE is a trademark of Synopsys, Inc.
Input File: example.sp
lic:
lic: FLEXlm:v5.12 USER:hspiceuser HOSTNAME:hspiceserv
+ HOSTID:8086420f PID:1459
lic: Using FLEXlm license file:
lic: /afs/rtp/product/distrib/bin/license/license.dat
lic: Checkout hspice; Encryption code: AC34CE559E01F6E05809
lic: License/Maintenance for hspice will expire on 14-apr+ 1999/1999.200
590
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
lic: 1(in_use)/10 FLOATING license(s) on SERVER hspiceserv
lic:
******
* example hspice netlist using a linear cmos amplifier
******
* netlist options
.option post probe brief nomod
* defined parameters
Opening plot unit=15
file=./example.pa0
****** HSPICE -98.4 (981215) 13:58:43
****** 01/08/1999 solaris ******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
*** parameter analog_voltage = 1.000E+00 ***
node
=voltage
node
=voltage
node
=voltage
+0:clamp= 2.6200 0:in
=0.
0:infilt= 2.6200
+0:inv1out =2.6200 0:inv2out=2.6199
0:vdd
=5.0000
Opening plot unit=15
file=./example.tr0
**warning** negative-mos conductance=1:mnmos iter=2
vds,vgs,vbs=
2.45
2.93
0.
gm,gds,gmbs,ids= -3.636E-05
1.744E-04 0. 1.598E-04
******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
falltime=3.9149E-08 targ=7.1916E-08
trig=3.2767E-08
*** HSPICE -- 98.4 (981215) 13:58:43
*** 01/08/1999 solaris ***
* example hspice netlist using a linear cmos amplifier
****** transient analysis tnom=25.000 temp=25.000 ******
*** parameter analog_voltage = 2.000E+00 ***
node
=voltage
node
=voltage
node
=voltage
+0:clamp=2.6200
0:in
=0.
0:infilt= 2.6200
+0:inv1out=2.6200 0:inv2out=2.6199 0:vdd
=5.0000
******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
falltime=1.5645E-08 targ=5.7994E-08
trig=4.2348E-08
HSPICE® Simulation and Analysis User Guide
Y-2006.03
591
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
**** HSPICE -98.4 (981215) 13:58:43
**** 01/08/1999 solaris ****
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
*** parameter analog_voltage = 3.000E+00 ***
node
=voltage
node
=voltage
node
=voltage
+0:clamp= 2.6200 0:in
= 0.
0:infilt= 2.6200
+0:inv1out=2.6200 0:inv2out=2.6199 0:vdd
= 5.0000
******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
falltime=1.1917E-08 targ=5.6075E-08
trig=4.4158E-08
****** HSPICE -- 98.4 (981215) 13:58:43
****** 01/08/1999 solaris ******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
*** parameter analog_voltage = 4.000E+00 ***
node
=voltage
node
=voltage
node
=voltage
+0:clamp= 2.6200 0:in
= 0.
0:infilt= 2.6200
+0:inv1out=2.6200 0:inv2out=2.6199 0:vdd
= 5.0000
******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
falltime=7.5424E-09 targ=5.3989E-08
trig=4.6447E-08
****** HSPICE -- 98.4 (981215) 13:58:43
****** 01/08/1999 solaris ******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
*** parameter analog_voltage = 5.000E+00 ***
node
=voltage
node
=voltage
node
=voltage
+0:clamp= 2.6200 0:in
= 0.
0:infilt= 2.6200
+0:inv1out=2.6200 0:inv2out=2.6199 0:vdd
= 5.0000
******
* example hspice netlist using a linear cmos amplifier
***** transient analysis tnom=25.000 temp=25.000 *****
falltime=6.1706E-09 targ=5.3242E-08
592
trig=4.7072E-08
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
meas_variable=falltime
mean=16.0848n
varian=1.802e-16
sigma=13.4237n
avgdev= 9.2256n
max =39.1488n
min
= 6.1706n
***** job concluded
****** HSPICE -- 98.4 (981215) 13:58:43
****** 01/08/1999 solaris ******
* example hspice netlist using a linear cmos amplifier
*** job statistics summary tnom=25.000 temp=25.000 ***
total memory used
155 kbytes
# nodes=8 # elements=14
# diodes=2 # bjts
=
0 # jfets =0 # mosfets=4
analysis
time
# points
tot. iter
conv.iter
op point
0.04
1
23
transient
4.71
505
9322
2624 rev=664
readin
0.03
errchk
0.01
setup
0.01
output
0.01
total cpu time
4.84 seconds
job started at 13:58:43 01/08/1999
job ended
at 13:58:50 01/08/1999
lic: Release hspice token(s)
HSPICE job example.sp completed.
Fri Jan 8 13:58:50 EST 1999
Example.pa0
1 xinv1.
2 xinv2.
Example.st0
***** HSPICE -98.4 (981215) 13:58:43
***** 01/08/1999 solaris
Input File: example.sp
lic: FLEXlm:v5.12 USER:hspiceuser HOSTNAME:hspiceserv
+ HOSTID:8086420f PID:1459
lic: Using FLEXlm license file:
lic: /afs/rtp/product/distrib/bin/license/license.dat
lic: Checkout hspice; Encryption code: AC34CE559E01F6E05809
lic: License/Maintenance for hspice will expire on
+ 14-apr-1999/1999.200
HSPICE® Simulation and Analysis User Guide
Y-2006.03
593
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
lic: 1(in_use)/10 FLOATING license(s) on SERVER hspiceserv
lic:
init: begin read circuit files, cpu clock=2.21E+00
option probe
option nomod
init: end read circuit files, cpu clock=2.23E+00
+ memory=145 kb
init: begin check errors, cpu clock=2.23E+00
init: end check errors, cpu clock=2.24E+00 memory=144 kb
init: begin setup matrix, pivot=
10 cpu clock=2.24E+00
establish matrix -- done, cpu clock=2.24E+00 memory=146 kb
re-order matrix -- done, cpu clock=2.24E+00 memory=146 kb
init: end setup matrix, cpu clock=2.25E+00 memory=154 kb
sweep: parameter parameter1
begin, #sweeps= 5
parameter: analog_voltage= 1.00E+00
dcop: begin dcop, cpu clock=2.25E+00
dcop: end dcop, cpu clock=2.27E+00 memory=154 kb
tot_iter=11
output: ./example.mt0
sweep: tran tran1 begin, stop_t=1.00E-06 #sweeps=101
cpu clock= 2.28E+00
tran: time=1.03750E-07 tot_iter=78
conv_iter=24
tran: time=2.03750E-07 tot_iter=179
conv_iter=53
tran: time=3.03750E-07 tot_iter=280
conv_iter=82
tran: time=4.03750E-07 tot_iter=381
conv_iter=111
tran: time=5.03750E-07 tot_iter=482
conv_iter=140
tran: time=6.03750E-07 tot_iter=583
conv_iter=169
tran: time=7.03750E-07 tot_iter=684
conv_iter=198
tran: time=8.03750E-07 tot_iter=785
conv_iter=227
tran: time=9.03750E-07 tot_iter=886
conv_iter=256
tran: time=1.00000E-06 tot_iter=987
conv_iter=285
sweep: tran tran1 end, cpu clock=2.82E+00 memory=155 kb
parameter: analog_voltage= 2.00E+00
dcop: begin dcop, cpu clock=2.83E+00
dcop: end dcop, cpu clock=2.83E+00 memory=155 kb
+ tot_iter=14
output: ./example.mt0
sweep: tran tran2 begin, stop_t=1.00E-06 #sweeps=101
+ cpu clock=2.83E+00
tran: time=1.01016E-07 tot_iter=186
conv_iter=54
tran: time=2.02642E-07 tot_iter=338
conv_iter=98
tran: time=3.01763E-07 tot_iter=495
conv_iter=145
tran: time=4.04254E-07 tot_iter=668
conv_iter=198
tran: time=5.02594E-07 tot_iter=841
conv_iter=248
tran: time=6.10102E-07 tot_iter=983
conv_iter=289
594
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
tran:
tran:
tran:
tran:
time=7.01850E-07
time=8.01776E-07
time=9.04268E-07
time=1.00000E-06
tot_iter=1161
tot_iter=1306
tot_iter=1481
tot_iter=1654
conv_iter=340
conv_iter=383
conv_iter=436
conv_iter=486
sweep: tran tran2 end, cpu clock=3.71E+00 memory=155 kb
parameter: analog_voltage= 3.00E+00
dcop: begin dcop, cpu clock=3.71E+00
dcop: end dcop, cpu clock=3.72E+00 memory=155 kb
+ tot_iter=17
output: ./example.mt0
sweep: tran tran3 begin, stop_t=1.00E-06 #sweeps=101
+ cpu clock=3.72E+00
tran: time=1.00313E-07 tot_iter=143
conv_iter=42
tran: time=2.01211E-07 tot_iter=340
conv_iter=100
tran: time=3.01801E-07 tot_iter=539
conv_iter=156
tran: time=4.02192E-07 tot_iter=729
conv_iter=211
tran: time=5.01997E-07 tot_iter=917
conv_iter=265
tran: time=6.01801E-07 tot_iter=1088
conv_iter=314
tran: time=7.01801E-07 tot_iter=1221
conv_iter=351
tran: time=8.01801E-07 tot_iter=1362
conv_iter=392
tran: time=9.02387E-07 tot_iter=1515
conv_iter=435
tran: time=1.00000E-06 tot_iter=1674
conv_iter=479
sweep: tran tran3 end, cpu clock=4.57E+00 memory=155 kb
parameter: analog_voltage= 4.00E+00
dcop: begin dcop, cpu clock=4.57E+00
output: ./example.mt0
sweep: tran tran4 begin, stop_t=1.00E-06 #sweeps=101
+ cpu clock=4.58E+00
tran: time=1.00110E-07 tot_iter=236
conv_iter=70
tran: time=2.04376E-07 tot_iter=475
conv_iter=139
tran: time=3.07892E-07 tot_iter=767
conv_iter=221
tran: time=4.01056E-07 tot_iter=951
conv_iter=273
tran: time=5.01086E-07 tot_iter=1250
conv_iter=353
tran: time=6.00965E-07 tot_iter=1541
conv_iter=432
tran: time=7.03668E-07 tot_iter=1805
conv_iter=506
tran: time=8.01114E-07 tot_iter=2046
conv_iter=571
tran: time=9.01005E-07 tot_iter=2308
conv_iter=640
tran: time=1.00000E-06 tot_iter=2528
conv_iter=703
sweep: tran tran4 end, cpu clock=5.83E+00 memory=155 kb
parameter: analog_voltage= 5.00E+00
dcop: begin dcop, cpu clock=5.83E+00
dcop: end dcop, cpu clock=5.84E+00 memory=155 kb
HSPICE® Simulation and Analysis User Guide
Y-2006.03
595
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
+ tot_iter=23
output: ./example.mt0
sweep: tran tran5 begin, stop_t=1.00E-06 #sweeps=101
+ cpu clock=5.84E+00
tran: time=1.00195E-07 tot_iter=176
conv_iter=47
tran: time=2.00617E-07 tot_iter=431
conv_iter=115
tran: time=3.00475E-07 tot_iter=661
conv_iter=176
tran: time=4.00719E-07 tot_iter=914
conv_iter=246
tran: time=5.04084E-07 tot_iter=1157
conv_iter=311
tran: time=6.00666E-07 tot_iter=1347
conv_iter=363
tran: time=7.01830E-07 tot_iter=1623
conv_iter=435
tran: time=8.02418E-07 tot_iter=1900
conv_iter=514
tran: time=9.01178E-07 tot_iter=2161
conv_iter=585
tran: time=1.00000E-06 tot_iter=2410
conv_iter=650
sweep: tran tran5 end, cpu clock=7.03E+00 memory=155 kb
sweep: parameter
parameter
1 end
>info:
***** hspice job concluded
lic: Release hspice token(s)
Simulation Graphical Output in AvanWaves
The plots in Figure 113 through Figure 118 on page 602 show the six different
post-processor outputs from the simulation of the example netlist. These plots
are postscript output from the actual data in AvanWaves, a Synopsys graphical
waveform viewer.
596
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Figure 113 Plot of Voltage on Node in
HSPICE® Simulation and Analysis User Guide
Y-2006.03
597
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Figure 114 Plot of Voltage on Node clamp vs. Time
598
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Figure 115 Plot of Voltage on Node inv1out vs.Time
HSPICE® Simulation and Analysis User Guide
Y-2006.03
599
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Figure 116 Plot of Voltage on Node inv2out vs. Time
600
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using AvanWaves
Figure 117 Plot of Current through Diode dlow vs. Time
HSPICE® Simulation and Analysis User Guide
Y-2006.03
601
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
Figure 118 Plot of Measured Variable falltime vs. Amplifier Input Voltage
Simulation Example Using CosmosScope
This example demonstrates the basic steps to perform simulation output and to
view the waveform results by using the Synopsys CosmosScope Waveform
Viewer.
Input Netlist and Circuit
This example is based on demonstration netlist bjtdiff.sp, which is available in
directory $<installdir>/demo/hspice/apps. This shows the input netlist for a BJT
diff amplifier. Comment lines indicate the individual sections of the netlists. See
the HSPICE Command Reference for information about individual commands.
*file: bjtdiff.spbjt diff amp with every analysis type
*
602
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
.options acct node list opts nomod post
.param rb1x=aunif(20k,1k,30k) rb2x=aunif(20k,1k,30k)
.tf v(5) vin
.dc vin -0.20 0.20 0.01 sweep monte=3
.ac dec 10 100k 10meghz
.noise v(4) vin 20
.net v(5) vin rout=10k
.pz v(5) vin
.disto rc1 20 .9 1m 1.0
.sens v(4)
.tran 5ns 200ns
.four 5meg v(5) v(15)
.temp -55 150
*
.meas qa_propdly trig v(1) val=0.09 rise=1
+ targ v(5) val=6.8 rise=1
.meas qa_magnitude max v(5)
.meas qa_rmspower rms power
.meas qa_avgv5 avg v(5)
.meas ac qa_bandwidth trig at=100k targ vdb(5) val=36 fall=1
.meas ac qa_phase find vp(5) when vm(5)=52.12
.meas ac qa_freq when vm(5)=52.12
.print dc v(4) v(5) v(14) v(15)
.probe dc v(5) v(15)
.print ac vm(5) vp(5) vm(15) vp(15)
.probe ac vm(5) vp(5) vm(15) vp(15)
.print ac vt(5) vt(15)
.probe noise onoise(m) inoise(m)
.print ac z11(m) z12(m) z22(m) zin(m)
.probe ac z11(p) z12(p) z22(p) zin(p)
.probe disto hd2 hd3 sim2 dim2 dim3
.print tran v(4) v(5) v(14) v(15)
.print tran p(vcc) p(vee) p(vin) power
.probe tran v(5) v(15)
*
vin 1 0 sin(0 0.1 5meg) ac 1
vcc 8 0 12
vee 9 0 -12
*
q1 4 2 6 qnl
q11 14 12 16 qpl
q2 5 3 6 qnl
q21 15 13 16 qpl
rs1 1 2 1k
rs11 1 12 1k
rs2 3 0 1k
rs12 13 0 1k
rc1 4 8 10k
HSPICE® Simulation and Analysis User Guide
Y-2006.03
603
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
rc11 14 9 10k
rc2 5 8 10k
rc12 15 9 10k
q3 6 7 9 qnl
q13 16 17 8 qpl
q4 7 7 9 qnl
q14 17 17 8 qpl
rb1 7 8 rb1x
rb2 17 9 rb2x
*
.model qnl npn(bf=80 rb=100 ccs=2pf tf=0.3ns tr=6ns cje=3pf
cjc=2pf
+ va=50 rc=10 trb=.005 trc=.005)
.model qpl pnp(bf=80 rb=100 ccs=2pf tf=0.3ns tr=6ns cje=3pf
cjc=2pf
+ va=50 bulk=0 rc=10)
*
.end
Use the previous example (linear CMOS amp) to draw a circuit diagram for this
BJT diff amplifier. Also, specify parameter values.
Execution and Output Files
This section displays the various output files from a HSPICE simulation of the
BJT diff amplifier example. To execute the simulation, enter:
hspice bjtdiff.sp > bjtdiff.lis
where the input file is bjtdiff.sp, and the output file is bjtdiff.lis.
604
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
Simulation creates the following output files:
Table 62
Output Files
Filename
Description
bjtdiff.ic
Initial conditions for the circuit.
bjtdiff.lis
Text simulation output listing.
bjtdiff.mt0
Post-processor output for .MEASURE statements.
bjtdiff.st0
Run-time statistics.
bjtdiff.tr0
Post-processor output for transient analysis.
bjtdiff.sw0
Post-processor output for DC analysis.
bjtdiff.ac0
Post-processor output for AC analysis.
bjtdiff.ma0
Post-processor output for AC analysis measurements.
View HSPICE Results in CosmosScope
The steps below show how to use the Synopsys CosmosScope Waveform
Viewer to view the results of AC, DC, and transient analysis from the BJT diff
amplifier simulation. Refer to previous examples of .lis, .ic, and .st0 files.
Viewing HSPICE Transient Analysis Waveforms
To view HSPICE transient analysis waveforms, do the following:
1. Invoke CosmosScope.
From a Unix command line, type:
% cscope
On a Windows-NT system, choose the menu command:
Programs > (user_install_location)> CosmosScope
2. Open the Open Plotfiles dialog box:
File > Open > Plotfiles
HSPICE® Simulation and Analysis User Guide
Y-2006.03
605
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
3. In the Open Plotfiles dialog box, in the Files of Type fields, select the Hspice
Transient (*.tr*) item.
4. In the menu, click on bjtdiff.tr0, and click Open.
The Signal Manager and the bjtdiff Plot File windows open.
5. Hold down the Ctrl key, and select the v(4), v(5), and ITPOWERD(power)
signals.
6. Click on Plot from the bjtdiff Plot File window.
Three cascaded plots open.
7. To see three signals in one plot, right-click on the top-most signal name.
The Signal Menu opens.
8. From the Signal Menu, select Stack Region > Analog 0.
9. Repeat Step 7 for the next topmost signal.
A plot opens similar the one shown in Figure 119 on page 607.
606
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
Figure 119 Transient Analysis: Plot of v(4), v(5), and ITPOWERD (power)
Viewing HSPICE AC Analysis Waveforms
To view HSPICE AC analysis waveforms, do the following:
1. From the Signal Manager dialog box, select bjtdiff(1), and click on Close
Plotfiles.
All transient plots (waveforms) close.
2. In the Signal Manager, click on Open Plotfiles.
3. In the Open Plotfiles dialog box, in the Files of Type fields, select the
HSPICE AC (*.ac*) item.
4. Click on bjtdiff.ac0 in the menu, and click Open.
The bjtdiff Plot File windows open.
5. Hold down the Ctrl key, and select the dim2(mag) and dim3(mag) signals.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
607
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
6. Click on Plot from the bjtdiff Plot File window.
Two cascaded plots open.
7. For two signals in a plot, right-click on dim2(mag).
A Signal Menu opens.
8. From the Signal Menu, select Stack Region > Analog 0.
A plot opens similar to Figure 120.
Figure 120 AC Analysis Result: Plot of dim2(mag), dim3(mag) from bjtdiff.ac0
608
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
Viewing HSPICE DC Analysis Waveforms
To view HSPICE DC analysis waveforms, do the following:
1. From the Signal Manager dialog box, select bjtdiff(1), and click on Close
Plotfiles.
All AC plots (waveforms) close.
2. In the Signal Manager, click on Open Plotfiles.
3. In the Open Plotfiles dialog, Files of Type field, select HSPICE DC (*.sw*).
4. Click on bjtdiff.sw0 and Open in the menu.
The Plot File windows open.
5. Hold down the Ctrl key and select all signals.
6. Click on Plot from the bjtdiff Plot File window.
Four cascaded plots open.
7. To see four signals in one plot, right-click on the name of the top-most signal.
A Signal Menu opens.
8. From the Signal Menu, select Stack Region > Analog 0.
9. Repeat Steps 7 and 8 for the next two top-most signals.
A plot opens similar to the one shown in Figure 121.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
609
Appendix B: Full Simulation Examples
Simulation Example Using CosmosScope
Figure 121 DC Analysis Result: Plot of v(14), v(15), v(4), and v(5) from
bjtdiff.sw0
The CosmosScope User’s and Reference Manual includes a full tutorial,
information about the various Scope tools, and reference information about the
Measure tool. You can also find more information on the Synopsys website:
http:// www.synopsys.com
610
HSPICE® Simulation and Analysis User Guide
Y-2006.03
C
C
HSPICE GUI for Windows
Describes how to use the HSPICE GUI for Windows.
To open and install the the GUI, click on the HSPUI icon. Figure 122 shows the
directory structure for the HSPICE GUI for Windows.
Figure 122 Directory Structure
Design dir
Sim. input
*.sp
Design Config
*.cfg
Raw output
.tr#,.ac#,.sw#
Measures
.mt#,.ma#,.ms#
Sim. output
.lis
Working with Designs
A new design can be created in several ways. The Launcher allows you to
browse for an input file for HSPICE, which has the default file suffix .sp. The
Launcher Browse button opens a standard file browser.
Selecting a file of the type <design>.sp causes the Launcher to display the
main form, which contains the following items:
■
input filename
■
design title (the first line of the file <design>.sp)
■
output filename
■
HSPICE and AvanWaves version
HSPICE® Simulation and Analysis User Guide
Y-2006.03
611
Appendix C: HSPICE GUI for Windows
Working with Designs
New designs can be saved with the command File > Save.
Table 63
Design Commands in the Launcher
Command
Description
File > New
Clears the Launcher and opens a new design
File > Open
Opens an existing design with the file browser
File > Save
Saves the current design information
File > Save As
Not implemented in Version 1.0
File > Close
Closes the current design
<LastDesigns>
Lists the last five designs opened
File > Exit
Exits the Launcher
The commands File > New, Open, and Close prompt you to save the current
design if changes have occurred.
The Launcher checks on the status of a given design when it is opened. If the
input file exists, the Simulate button is active. If the listing file exists for the
design, the Edit Listing button is active. The Edit Netlist and AvanWaves
buttons are always active.
You do not need to save a design to Simulate or view the results of a simulation
with AvanWaves.
Figure 123 shows the main window of the Launcher.
612
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix C: HSPICE GUI for Windows
Configuring the HSPICE GUI for Windows
Figure 123 Launcher Main Window
Configuring the HSPICE GUI for Windows
Customize configurations using the Configuration menu of the Launcher as
shown in Figure 124.
The start-up directory defaults to the value of the AVANHOME environment
variable set up during HSPICE installation.
■
The input file suffix defaults to .sp.
■
The output file suffix defaults to .lis.
■
The editor defaults to notepad.exe.
If you change a value, the Launcher updates the <AVANHOME>/hspui.cfg file.
The next Launcher run provides the new values.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
613
Appendix C: HSPICE GUI for Windows
Running Multiple Simulations
Figure 124 Launcher Options Window
The Configuration > Versions item lists current executables and their paths for
the Launcher (HSPUI), HSPICE, and AvanWaves.
Note:
Standard menu items, such as File and Edit, display on the HSPICE/Win
menu bar, but are not available in this release. The Configuration > Version
strings change from the main window Versions combo box. You cannot
change them here.
To associate your <design>.sp file with the Launcher, use the File >> Associate
command in the Windows File Manager. You can double-click on an .sp file in
the File Manager window to automatically invoke the HSPICE/Win Launcher.
Refer to your Windows documentation for details on how to do this.
Running Multiple Simulations
Use the HSPICE/Launcher file browser to build a list of simulations from
different directories for consecutive HSPICE processing.
Press Multi-Jobs in the main window to open the HSPICE Multi-Job window
(Figure 125). Simulation files are chosen from the Drive/Directory list box and
placed in the Files list box.
614
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Appendix C: HSPICE GUI for Windows
Running Multiple Simulations
Figure 125 HSPICE Multi-Jobs Window
Building the Batch Job List
To build a batch job list:
1. Press Multi-Jobs in the main window.
2. Using the Drive/Directory boxes, locate the directory of files that you wish to
simulate.
3. To copy all files in the directory, press the Copy button on the right side of
the Hspbat window.
Note that any file names already in the list will be replaced.
4. To add additional files from other directories, repeat Step 2 and use the
Append button.
HSPICE® Simulation and Analysis User Guide
Y-2006.03
615
Appendix C: HSPICE GUI for Windows
Running Multiple Simulations
Simulating the Batch Job List
To simulate a batch job list:
1. To simulate all of the files in the Batch Job list, set the pulldown menu to All
and press the Simulate button.
2. To run simulation on a single file or a group of files, set the pulldown menu
to Selected and select those files you wish to simulate from the Batch Job
list box.
Use the left mouse button to select a single file.
•
Press and hold the Control key and select another file with the left
mouse button to add to the selected list.
•
Press and hold the Shift key to select all files between the current file
and the last selected file.
3. Press the Simulate button to start the consecutive simulations.
Using the Drag-and-drop Functions
The HSPICE Multi-Jobs window provides a drag-and -rop capability to remove
files from the list, edit files, run simulations and view the results with
AvanWaves.
Beside the icons, the user also can use the Text Editor box to view and edit the
design file (<design>.sp). To do this, drag and drop the file from the upper list
box to the bottom one. The file contents are displayed in the bottom editor for
the user to view and/or edit.
To display files associated with a design, double click on the upper list box on
the selected design file (<design>.sp file). All associated files (tr#, ac#, sw#,
mt# ...) are listed in the bottom list box.
616
HSPICE® Simulation and Analysis User Guide
Y-2006.03
Index
Symbols
!GND node 47
$installdir installation directory 61
A
A2D
function 199
model parameter 199
output model parameters 203
See also mixed mode
.a2d file 15, 17, 199
ABS element parameter 196
abs(x) function 229
ABSI option 298
ABSMOS option 298
absolute
power function 229
value function 229
value parameter 196
ABSV option 298
ABSVAR option 328
AC analysis 243
output 260
RC network 346
resistance 345
small signals 344
sources 123
AC analysis measurement results file 16
AC analysis results file 16
AC choke inductors 87
.AC statement 469, 547
.ac# file 15, 16
accuracy
control options 299
simulation time 299
tolerance 297, 298, 327
ACCURATE option 328
ACM model parameter 329
acos(x) function 229
ACOUT option 262–263
adder
circuit 507
demo 506
NAND gate binary 508
subcircuit 507
admittance
AC input 265
AC output 265
Y parameters 260
AF model parameter 350
AGAUSS keyword 557
algebraic
expressions 228
models 329
algorithm
linear acceleration 500
numerical integration 333
algorithms
Damped Pseudo Transient algorithm 307
DVDT 334, 335
GEAR 330
integration 330
iteration count 334
Levenberg-Marquardt 478
local truncation error 334
timestep control 333, 334, 335
trapezoidal integration 330
.ALTER
blocks 53
statement 54, 55, 249
AM
source function 145, 145–146
analog transition data file 15
analyses
Monte Carlo 445
analysis
AC 243
accuracy 297–299
data driven 545
DC 243
element template 243
617
Index
B
Fourier 338
initialization 288
inverter 320
.MEASURE statement 243
Monte Carlo 545, 553, 553–577
optimization 469
parametric 243
RC network 318, 346
statistical 548–577
Taguchi 544
temperature 544, 547
transient 243, 316
worst case 544, 548–577
yield 544
arccos(x) function 229
arcsin(x) function 229
arctan(x) function 229
arithmetic operators 229
ASIC libraries 62
asin(x) function 229
atan(x) function 229
ATEM characterization system 61
AUNIF keyword 557
autoconvergence 302
AUTOSTOP option 327
average deviation 545
average value, measuring 271
B
B# node name in CSOS 49
backslash continuation character 228
batch job list, MS Windows launcher 615
behavioral
current source 186
voltage source 171
Behavioral capacitors 76
Behavioral resistors 69
Biaschk 321
Bipolar Junction Transistors. See BJTs
BJTs
current flow 255
element template listings 279
elements, names 93
power dissipation 258
S-parameters, optimization 485
bond wire example 513
618
branch current
output 253
breakpoint table
reducing size 337
buffer 118
C
C Element (capacitor) 74
calculating 28
calculating new measurements
new measurements 28
capacitance
element parameter 71
manufacturing variations 566
capacitor
conductance requirement 306
current flow 254
element 71, 74, 275
frequency-dependent 75
linear 74
models 71
voltage controlled 188, 193
CAPOP model parameter 329
CCCS element parameter 180
CCVS element parameter 195, 196
cell characterization 545
characterization of models 295
CHGTOL option 335
circuits
adder 507
description syntax 39
inverter, MOS 320
nonconvergent 310
RC network 346
reusable 57
subcircuit numbers 48
temperature 547
See also subcircuits
client/server mode 26
client 27
quitting 28
server 26
simulating 27
starting 26
CLOAD model parameter 203
CMOS
output driver demo 513
tristate buffer, optimization 481
Index
D
commands
hspice 20
hspice -I 23
hspicerf 22
limit descriptors 249
output 241
comment line
netlist 40
VEC files 218
common emitter gain 520
compression of input files 29
conductance
for capacitors 306
pn junction 313
configuration
MS Windows launcher 613
configuration file 14
continuation character, parameter strings 228
continuation of line
netlist 41
control options
accuracy 299
defaults 336
algorithm selection 296
convergence 296, 300
DC convergence 297
initialization 296
method 325
printing 248
transient analysis
method 325–326
controlled sources 156, 158
CONVERGE option 301, 307
convergence
control options 300
problems 307
analyzing 308
autoconverge process 302
causes 310
CONVERGE option 307
DCON setting 302
diagnosing 307–313
diagnostic tables 308
floating point overflow 307
GMINDC ramping 302
.NODESET statement 293
reducing 304
cos(x) function 229
cosh(x) function 229
current
branch 254
controlled
current sources 157, 180, 277
voltage sources 157, 195, 278
in HSPICE elements 254
output 252
sources 184
C-V plots 509
D
D2A
function 199
input model parameters 200
model parameter 199
See also mixed mode
.d2a file 199
Damped Pseudo Transient algorithm 307
data
flow, overview 7
.DATA statement 50
data-driven analysis 50
data type definitions 359
data-driven analysis 545
PWL source function 143
db(x) function 230
DC
analysis 242, 296–297
capacitor conductances 306
initialization 296
convergence control options 296, 297
errors, reducing 304
operating point
analysis 291
bypassing 317
initial conditions file 14
See also operating point
sources 123
sweep 295
DC analysis measurement results file 17
DC analysis results file 17
.DC statement 295, 469, 547
DCCAP option 508
.DCMATCH output tables file 19
DCON option 301, 302
DCSTEP option 306
619
Index
D
.DCVOLT statement 293
DDL 61, 520
DDLPATH environment variable 61, 520
decibel function 230
DEFAULT_INCLUDE variable 14
definitions
data types 359
DEFW option 236
.DEL LIB statement 36
in .ALTER blocks 53
with .ALTER 55
with .LIB 55
with multiple .ALTER statements 54
DELAY element parameter 190, 196
delays
element example 193
group 264
time (TD) 264
DELMAX option 328, 336, 340
DELTA
element parameter 190, 196
DELVTO model parameter 549
demo files
2n2222 BJTs transistor characterization 533
2n3330 JFETs transistor characterization 532
A/D flash converter 529
A2D 529
AC analysis 525
acl gate 526
adders
72-transistor two-bit 527
BJT NAND gate two-bit 526
BJT two-bit 525
D2A 529
MOS two-bit 526
NAND gate four-bit binary 525
air core transformer 536
algebraic
output variables 524–525
parameters 524
transmission lines 540
.ALTER statement 525
AM source 539
amplifier 529
amplitude modulator 526
analog 528
AND gate 526
automatic model selection program 537
620
behavioral applications 526–527
behavioral models 528
diode 526
D-latch 526
filter 524
NAND gate 527
ring oscillator 527
triode 527
voltage to frequency converter 524
benchmarks 527–528
bisection 528
BJTs
analog circuit 528
beta plot 528
differential amplifier 525, 529
diodes 528
ft plot 528
gm, gpi plots 528
photocurrent 538
Schmidt trigger 525
sense amplifier 525
BSIM3 model, LEVEL=47 536
capacitances, MOS models
LEVEL=13 536
LEVEL=2 536
LEVEL=6 536
cell characterization 525, 526, 528–529
charge conservation, MOS models
LEVEL=3 536
LEVEL=6 537
circuit optimization 529
CMOS
differential amplifier 525
I/O driver ground bounce 525, 540
input buffer 529
inverter macro 527
output buffer 529
coax transmission line 540
crystal oscillator 525
current controlled
current source 527
voltage source 527
D2A 529
DC analysis, MOS model LEVEL=34 537
DDL 529–533
delay 525, 528, 529
device optimization 533
differential amplifier 525
differentiator 526
Index
D
diffusion effects 525
diode photocurrent 538
D-latch 526
E Element 526
edge triggered flip-flop 526
exponential source 539
FFT
AM source 533
analysis 533–535
Bartlett window 534
Blackman window 534
Blackman-Harris window 534
data-driven transient analysis 534
exponential source 534
Gaussian window 534
Hamming window 534
Hanning window 534
harmonic distortion 534
high frequency detection 534
intermodulation distortion 534
Kaiser window 534
modulated pulse source 534
Monte Carlo, Gaussian distribution 534
product of waveforms 534
pulse source 534
PWL 535
rectangular window 535
single-frequency FM source 535
sinusoidal source 534
small-signal distortion 534
switched capacitor 535
transient 534
window tests 535
filter matching 529
filters 535–536
behavioral 524
fifth-order 527, 535
fourth-order Butterworth 535
Kerwin’s circuit 535
LCR bandpass 535
matching lossy to ideal 529
ninth-order low-pass 526, 535
switched capacitor low-pass 526
FR-4 microstrip transmission line 536, 539
G Element 525, 526
GaAsFET amplifier 525
gamma model LEVEL=6 537
general applications 525–526
ground bounce 525, 540
group time delay 525
impact ionization plot 536
input 524
installation test 527
integrator 526
inverter 525, 526, 527, 528
characterization 528
IRF340 NMOS transistor characterization 532
I-V plots
LEVEL=3 537
MOSFETS model LEVEL=13 536
SOSFETS model LEVEL=27 537
JFETs photocurrent 539
junction tunnel diode 528
LCR circuit 529
lumped
MOS model 525
transmission lines 536, 540
magnetic core transformer 536
magnetics 536
microstrip transmission lines 535, 540
coupled 540
optimization 540
series 540
Monte Carlo analysis 525
Gaussian distribution 525
limit function 525
uniform distribution 525
MOS 527, 529
MOSFETs 536–537
sigma sweep 529
sweep 525
NAND gate 526, 527
NMOS E-mode model, LEVEL=8 539
noise analysis 525
op-amp 525, 526
characterization 530–532
voltage follower 527, 539
optimization 526
2n3947 Gummel model 533
DC 533
diode 533
GaAs 533
group delay 529
Hfe 533
I-V 533
JFETs 533
LEVEL=2 model beta 533
621
Index
D
LEVEL=28 533
MOS 533
s-parameter 533
speed, power, area 529
width 529
parameters 524
phase
detector 526
locked loop 526
photocurrent 537–539
GaAs device 539
photolithographic effects 525
pll 526
pole/zero analysis 525, 535
pulse source 539
PWL 539
CCCS 527
CCVS 527
switch element 527
VCCS 526, 527
VCO 527
VCVS 527
radiation effects 537–539
bipolar devices 537
DC I-V, JFETs 539
GaAs differential amplifier 539
JFETs devices 537–538
MOSFETs devices 538
NMOS 539
RC circuit optimization 529
resistor temperature coefficients 529
RG58/AU coax test 535
ring oscillator 527
Royer magnetic core oscillator 536
Schmidt trigger 525
sense amplifier 525
series source coupled transmission lines 540
setup 528
characterization 529
shunt terminated transmission lines 540
silicon controlled rectifier 527
sine wave sampling 526, 527
single-frequency FM source 539
sinusoidal source 539
skew models 526
SNAP to HSPICE conversion 528
sources 539
s-parameters 528, 535, 536
622
sweep 525
switch 526
switched capacitor 526, 527, 539
temperature effects
LEVEL=13 536
LEVEL=6 536
timing analysis 528
total radiation dose 538
transient analysis 525
transistor characterization 532
transmission lines 539–540
triode model 527
tunnel diodes 527, 528
twinlead transmission line model 540
U models 540
unity gain frequency 529
verilog-a 540–541
Viewsim
A2D input 529
D2A input 529
voltage follower 527
voltage-controlled
current source 526, 527
oscillator 524, 527
resistor inverter 539
voltage source 527
voltage-to-frequency converter 524
voltage-variable capacitor 526
waveform smoothing 527
worst case skew model 526
derivative, measuring 270
design
name 13
deviation, average 545
device characterization 61
diagnostic tables 308–309
digital
files 199
vector file 210
digital output file 17
digital vector file
Waveform Characteristics section 216
DIM2
parameter 266
DIM3
parameter 266
diodes
breakdown example 194
current flow 254
Index
E
elements 278
equations 193
junction 92
models 91
polysilicon capacitor length 92
power dissipation 257
directories
installation directory 61
TEMP 21
TMP 21
tmp 21
directory
structure 611
distortion 266
.dm# file 19
.DOUT statement 213
.dp# file 16
DTEMP parameter 519, 546, 547
DV option 302
DVDT
algorithm 330, 334
option 328, 334, 335
dynamic timestep algorithm 335
E
E Elements
applications 157
element multiplier 175
syntax statements 165
temperature coefficients 175
time delay keyword 175
editor, notepad.exe 613
electrical measurements 520
element
active
BJTs 93
diodes 91
JFETs 95
MESFETs 95
MOSFETs 97
C (capacitor) 74
IC parameter 292
identifiers 33
independent source 119, 129
L (inductor) 85
markers, mutual inductors 81
names 47
OFF parameter 290
parameters See element parameters 65
passive
capacitors 71
inductor 78
mutual inductor 81
resistors 65
R (resistor) 68
statements 41, 61
current output 253
independent sources 120
Laplace 167
pole/zero 168
temperature 547
templates 266–286
analysis 243
BJTs 279
capacitor 275
current-controlled 277
function 231
independent 278
inductor 276
JFETs 281
MOSFETs 283
mutual inductor 276
resistor 275
saturable core 286
voltage-controlled 276, 277
transmission line 101, 105, 109
voltage-controlled 156
element parameters
.ALTER blocks 53
BJTs 93–94
623
Index
F
PWL 139, 143
resistors 66–67
transmission lines
T Element 106
U Element 109
W Element 101, 102
.END statement
for multiple HSPICE runs 55
in libraries 51
location 55
missing 29
with .ALTER 54
.ENDL statement 51
environment
variable, METAHOME 613
environment variables 11, 61, 520
LM_LICENSE_FILE 11
META_QUEUE 11, 12
[email protected] 12
TEMP 21
TMP 21
tmpdir 21
equations 270, 272
ERR function 272
ERR1 function 272, 467
ERR2 function 273
ERR3 function 273
errors
cannot open
output spool file 249
DC 304
digital file has blank first line 199
file open 21
functions 272–273
internal timestep too small 291, 311, 317
missing .END statement 29
no DC path to ground 306
no input data 21
parameter name conflict 269
system resource inaccessible 249
example
AC analysis 262, 346
comment line 41
digital vector file 220
experiments 6
HSPICE vs. SPICE methods 262
Monte Carlo 560, 568
network analysis, bipolar transistor 385
624
optimization 470
transient analysis 318, 320
worst case 568
EXP source function
fall time 136
initial value 136
pulsed value 136
rise time 136
exp(x) function 230
experiment 6
exponential function 136, 230
expressions, algebraic 228
external data files 37
F
F Elements
applications 157
multiply parameter 181
syntax statements 180
time delay keyword 182
value multiplier 182
fall time
EXP source function 136
FAST option 327
FFT analysis graph data file 17
file
analog transition data 15
DC operating point initial conditions 14
hspui.cfg 613
initialization 14
input netlist 15
library input 15
.lis 613
netlist 611, 613
output configuration 14
output listing 613
.sp 611, 613
file descriptors limit 249
files
.a2d 15, 199
AC analysis measurement results 16
AC analysis results 16
.ac# 15
.d2a 199
DC analysis measurement results 17
DC analysis results 17
digital output 17
Index
G
external data 37, 50
FFT analysis graph data 17, 19
.ft# 15
.gr# 16
graph data 9
hardcopy graph data 17
hspice.ini 61
.ic 16, 290
include files 37
including 14
input 9
limit on number 249
.lis 16
.ma# 15
.ms# 15
.mt# 16
multiple simulation runs 55
names 13
operating point node voltages 18
output
listing 18
status 19
.pa# 16
scratch files 21
.st# 16
subcircuit cross-listing 19
.sw# 15
.tr# 16
transient analysis measurement results 17, 19
transient analysis results 19
files, output 15
FIND keyword 270
first character descriptions 31
Foster pole-residue form
E element 170
G element 170
Fourier
analysis 338
coefficients 340
equation 340
FREQ
function 169
model parameter 246
frequency
response
table 169, 185
variable 233
frequency table model 116
frequency-dependent
capacitor 75
inductor 86
FS option 336
FT option 335, 336
.ft# file 15, 17
functions
A2D 199
built-in 229–233
D2A 199
DERIVATIVE 271
ERR 272
INTEG 271
LAPLACE 167, 185
NPWL 189
POLE 168, 185
PPWL 189
table 229
See also independent sources
G
G Elements
applications 157
controlling voltages 190, 192
current 190
curve smoothing 191
element value multiplier 191
gate type 190
initial conditions 190
multiply parameter 190
names 190
polynomial 191
resistance 190
syntax statements 184
time delay keyword 192
transconductance 192
voltage to resistance factor 192
GaAsFET model DC optimization 489
gain, calculating 262
GAUSS
functions 562
keyword 557
parameter distribution 553
GEAR algorithm 330
global parameters 234
GMIN option 313
GMINDC option 302, 313
GND node 47
625
Index
H
GOAL keyword 467
.gr# file 16, 17
GRAMP
option 302, 305
.GRAPH statement 242, 245, 249, 509
graphical user interface. See GUI. 611
ground, node name 47
GUI
using 611–??
Gxxx element parameters 190
H
H Elements
applications 158
controlling voltage 197
data points 197
element multiplier 197
element name 196
gate type 196
initial conditions 196
maximum current 196
minimum current 196
syntax statements 195
time delay keyword 197
transresistance 197
H parameters 384
hardcopy graph data file 17
HD2 distortion 266
HD3 distortion 266
hertz variable 233
hierarchical designs, flattened 37
HSPICE
input netlist 611, 613
installation directory 61
starting 20
version
95.3 compatibility 336
hspice command 20
hspice -I command 23
hspice.ini file 61
hspicerf command 22
hspui.cfg 613
hybrid (H) parameters 260
hybrid parameter calculations 359
626
I
IBIS buffers 118
.ic file 16, 290
IC parameter 190, 196, 292, 293
.IC statement 288, 290, 293
from .SAVE 295
.ic# file 18
ideal
current sources 305
delay elements 157, 158, 328
op-amp 157, 172, 176
transformer 157, 172, 177
IDELAY statement 216
imaginary
part of AC voltage 262–263
impedance
AC 265
Z parameters 260
include files 14
.INCLUDE statement 36, 53, 62, 63
independent sources
AC 120, 123
AM function 145
current 120, 278
data driven PWL function 142
DC 120, 123
elements 120
EXP function 136
functions 129
mixed types 124
PULSE function 129
PWL function 139
SFFM function 143
SIN function 133
transient 120, 124
types 129
voltage 120, 278
See also sources
individual element temperature 547
inductor
frequency-dependent 86
inductors
AC choke 87
current flow 254
element 78, 276
node names 78
power-line 87
initial conditions 289
Index
J
file 14
statement 293
initialization 288, 290
file 14
saved operating point 294
initialization file 14
INOISE parameter 266
input
admittance 265
analog transition data file 15
data
adding library data 55
for data driven analysis 50
DC operating point initial conditions file 14
files
analog transition data 15
character case 30
compression 29
DC operating point 14
demonstration 524
initialization 14
library 15
names 13
netlist 15, 29
output configuration file 14
structure 36
table of components 37
impedance 265
initialization file 14
library file 15
netlist 39
netlist file
See also input files
15, 39–55, 587
output configuration file 14
input netlist file 15
input stimuli 274
input syntax
Monte Carlo 448
input/output
cell modeling 521
installation directory $installdir 61
int(x) function 230
integer function 230
integration
algorithms 330
interactive mode 23
quitting 24
running command files 24
starting 23
internal
nodes, referencing 48
interstage gain 262
inverter
analysis, transient 320
circuit, MOS 320
invoking
hspice 20
hspicerf 22
interactively 23
iterations
algorithm 332
count algorithm 334
number 479
I-V and C-V plotting demo 508
J
JFETs
current flow 255
elements 95, 281
length 96
power dissipation 259
width 96
K
keywords
analysis statement syntax 469
DTEMP 546
ERR1 467
GOAL 467
LAST 270
MONTE 554
optimization syntax 468
PAR 228
power output 257
PP 271
source functions 120
KF model parameter 350
L
L Element (inductor) 85
LA_FREQ option 502
LA_MAXR option 502
LA_MINC option 502
627
Index
M
LA_TIME option 502
LA_TOL option 502
Laplace
function 167, 185
transform 167, 185
frequency 169, 185
LAST keyword 270
launcher
MS Windows 611
leadframe example 513
LENGTH model parameter 564
Levenberg-Marquardt algorithm 478
.LIB
call statement 51
statement 36, 63
in .ALTER blocks 51, 53
with .DEL LIB 55
with multiple .ALTER statements 54
libraries
adding with .LIB 55
ASIC cells 62
building 51
configuring 236
creating parameters 234
DDL 61
duplicated parameter names 234
.END statement 51
integrity 234
search 62
selecting 51
subcircuits 63
vendor 62
library input file 15
limit descriptors command 249
LIMIT keyword 557
line continuation
VEC files 218
linear
acceleration 499
capacitor 74
inductor 85
matrix reduction 499
resistor 68
.lis file 16, 18
.lis file 613
listing file 613
LM_LICENSE_FILE environment variable 11
LMAX model parameter 5
628
LMIN model parameter 5
.LOAD statement 294
local
parameters 234
truncation error algorithm 334
log(x) function 230
log10(x) function 230
logarithm function 230
LV 267
LV18 model parameter 509
LVLTIM option 328, 334, 335
LX 267
LX7 model parameter 509
LX8 model parameter 509
LX9 model parameter 509
M
M element parameter 181, 190
.ma# file 15, 16
macros 55
magnitude
AC voltage 263
magnitude, AC voltage 260, 262
manufacturing tolerances 563
Marquardt scaling parameter 478
MAX parameter 190, 196
max(x,y) function 230
maximum value, measuring 271
mean, statistical 545
.MEASURE statement 242, 243, 269
expression 270
failure message 268
parameters 227
measuring parameter types 269
menu configuration, MS Windows launcher 613
MESFETs 95
META_QUEUE environment variable 11, 12
Meyer and Charge Conservation parameters 285
MIN parameter 190, 196
min(x,y) function 230
minimum
value, measuring 271
mixed mode
See also D2A, A2D
mixed sources 124
MODEL keyword 469
Index
N
model parameters
A2D 199
.ALTER blocks 53
capacitance distribution 566
D2A 199, 200–201
DELVTO 549
DTEMP 547
.GRAPH statement parameters 246
LENGTH 564
manufacturing tolerances 563
MONO 246
output 246
PHOTO 564
RSH 549
sigma deviations, worst case analysis 549
skew 548
TEMP 50, 547
temperature analysis 547
TIC 246
TOX 549
TREF 545, 547, 548
XPHOTO 565
model parameters See model parameters diodes
.MODEL statement 547
for .GRAPH 246
models
algebraic 329
characterization 295
DTEMP parameter 519
LV18 509
LX7, LX8, LX9 509
Monte Carlo analysis 553, 559, 568
reference temperature 547
specifying 62
typical set 552
MONO model parameter 246
Monte Carlo
analysis 445, 544, 545, 568–577
demo files 525
distribution options 556–558
application considerations 453
input syntax 448
simulation output 451
variation block options 450
MONTE keyword 554
MOS
inverter circuit 320
op-amp optimization 493
MOSFETs
current flow 255
drain diffusion area 98
elements 97, 283
initial conditions 98
node names 97
perimeter 98
power dissipation 259
source 98, 99
squares 98
temperature differential 99
zero-bias voltage threshold shift 99
MS Windows launcher 611
batch job list 615
multi jobs 614
.ms# file 15, 17
.mt# file 16, 17, 19
multiple .ALTER statements 54
multiply parameter 58, 67, 120
multipoint experiment 6
multithreading 24
mutual inductor 81, 276
N
NAND gate adder 508
natural
log function 230
NDIM 158
.NET parameter analysis 382
netlist 37
file example 39
flat 37
input files 29
schematic 37
structure 39
netlist file
example 39
network output 265, 387
nodal voltage output 252, 261
nodes
connection requirements 47
floating supply 48
internal 48
MOSFET’s substrate 48
names 44, 47, 49, 509
automatic generation 49
ground node 47
period in 45
629
Index
O
subcircuits 47, 48
zeros in 49
numbers 44, 47
phase or magnitude difference 262
shorted 306
terminators 48
.NODESET statement 288
DC operating point initialization 293
from .SAVE 295
noise
calculations 349
input 266
output 266, 349
noise parameters 358
norm of the gradient 478
notepad.exe 613
NPDELAY element parameter 197
NPWL function 189
numerical integration 333
O
ODELAY statement 216
OFF parameter 290
one-dimensional function 158
ONOISE parameter 266
.OP statement 291, 317
op-amps
open loops 305
optimization 493
operating point
estimate 291, 317
.IC statement initialization 293
initial conditions 14
.NODESET statement initialization 293
restoring 295
saving 49, 294
solution 289, 290
transient 317
630
Index
P
AC analysis measurement results file 16
AC analysis results file 16
admittance 265
commands 241
current 252
DC analysis measurement results file 17
DC analysis results file 17
.DCMATCH output tables file 19
digital output file 17
driver example 513
FFT analysis graph data file 17
files
AC analysis measurement results 16
AC analysis results 16
DC analysis measurement results 17
DC analysis results 17
.DCMATCH output tables file 19
digital output 17
FFT analysis graph data 17
hardcopy data 17
names 13
operating point information 17
operating point node voltages 18
output listing 18
output status 19
redirecting 13
subcircuit cross-listing 19
transient analysis measurement results 19
transient analysis results 19
graphing 246
hardcopy graph data file 17
impedance 265
network 265
nodal voltage, AC 261
noise 266, 349
operating point information file 17
operating point node voltages file 18
output listing file 18
output status file 19
parameters 251
power 256
printing 249–251
reusing 274
saving 245
statements 241
subcircuit cross-listing file 19
transient analysis measurement results file 19
transient analysis results file 19
variables 242
AC formats 263
function 231
voltage 252
output configuration file 14
output files 15
output listing file 18, 613
output status file 19
overview of data flow 7
overview of simulation process 9
P
.pa# file 16, 19
packed input files 29
PAR keyword 228
.PARAM statement 52, 269, 544
in .ALTER blocks 53
parameter analysis, .NET 382
parameters
ACM 329
admittance (Y) 260
AF 350
algebraic 228, 229
analysis 227
assignment 225
CAPOP 329
cell geometry 233
constants 226
data type 225
data-driven analysis 50
defaults 238
defining 223, 234
DIM2 266
DIM3 266
evaluation order 225
HD2 266
HD3 266
hierarchical 58, 233, 269–270
hybrid (H) 260
IC 293
impedance (Z) 260
inheritance 236, 238
INOISE 266
input netlist file 36
KF 350
libraries 234–236
M 58
631
Index
P
measurement 227
model 200, 203
modifying 50
multiply 227
ONOISE 266
optimization 233
OPTxxx 467, 468
output 251
overriding 235, 238
PARHIER option 238
passing 233–240
order 225
problems 240
Release 95.1 and earlier 240
repeated 269
scattering (S) 260
scope 233–234, 240
SIM2 266
simple 226
subcircuit 58
two-port noise 358
user-defined 226
UTRA 304
parametric analysis 243
PARHIER option 238
path names 48
peak-to-peak value, measuring 271
phase
AC voltage 262–263
calculating 262
PHOTO model parameter 564
PI (linear acceleration) algorithm 501
piecewise linear sources See PWL
pivot
selection 326
PIVOT option 326
plot limits 244
.PLOT statement 242
simulation results 244, 249
pn junction conductance 313
POLE
function 168, 185
transconductance element statement 168
voltage gain element statement 168
pole/zero
conjugate pairs 168
function, Laplace transform 168, 185
POLY parameter 158, 191, 197
632
polynomial function 158
one-dimensional 158
three-dimensional 160
two-dimensional 159
[email protected] environment variable 12
POST option 9
pow(x,y) function 229
power
dissipation 256, 260
function 229
output 256
stored 256
POWER keyword 257
power-line inductors 87
PP keyword 271
PPWL
element parameter 191
function 189
print
control options 248
.PRINT statement 242
simulation results 243, 249
printer, device specification 246
.PROBE statement 242, 245, 249
program structure 5
PRTDEFAULT printer 246
PULSE source function 130, 133, 136, 139
delay time 130
initial value 130
onset ramp duration 130
plateau value 130
recovery ramp duration 130
repetition period 130
width 130
PUTMEAS option 268
PWL
current controlled gates 157, 158
data driven 142
element parameter 182, 191, 197
functions 158, 162
gates 157
output values 139
parameters 139
repeat parameter 139
segment time values 139
simulation time 337
sources, data driven 142
Index
Q
voltage-controlled capacitors 157
voltage-controlled gates 157
See also data driven PWL source
pwr(x,y) function 229
.PZ statement 296
Q
quality assurance 544
R
R Element (resistor) 68
RC
analysis 318, 346
circuit 346
optimizing 476
rcells, reusing 234
real part of AC voltage 262–263
reference temperature 50, 547
RELI option 298
RELMOS option 298, 328
RELQ option 335
reluctors 88
RELV option 298
RELVAR option 328
repeat function 506
residual sum of squares 478
resistance 345
resistor
current flow 254
element 66
element template listings 275
length parameter 67
linear 68
model name 66
node to bulk capacitance 67
voltage controlled 187
width parameter 67
reusing simulation output 274
RLOAD model parameter 203
RMAX option 336
RMIN option 336
rms value, measuring 271
RSH model parameter 549
S
S19NAME model parameter 204
S19VHI model parameter 204
S19VLO model parameter 204
S1NAME model parameter 204
S1VHI model parameter 204
S1VLO model parameter 204
saturable core
elements 81, 82, 286
models 80, 82
winding names 286
.SAVE statement 294
scale factors 34
SCALE parameter 66, 175, 182, 191, 197, 508
scaling, effect on delays 522
scattering (S) parameters 260
schematic
netlists 37
scope of parameters 234
scratch files 21
SEARCH option 63, 520
search path, setting 51
.SENS statement 296
SFFM source function
carrier frequency 144
modulation index 144
output amplitude 144
output offset 144
signal frequency 144
sgn(x) function 230
shorted nodes 306
sign function 230
SIGNAME element parameter 203
signed power function 229
silicon-on-sapphire devices 49
SIM_ANALOG option 87
SIM_LA option 499, 502
SIM_RAIL option 87
SIM2 distortion measure 266
simulate button 612
simulation
ABSVAR option 336
accuracy 327, 466
models 329
option 329, 336
timestep 328
633
Index
S
tolerances 297, 298, 327
electrical measurements 520
example 587
graphical output 596
multiple runs 55
performance, multithreading 24
process, overview 9
reducing time 337
results
graphing 246
printing 249–251
specifying 269–270
reusing output 274
speed 327
structure 5
time, RELVAR option 336
title 40
simulation output
Monte Carlo 451
SIN source function 133
sin(x) function 229
single point experiment 6
single-frequency FM source function 143
sinh(x) function 229
sinusoidal source function 133
skew
file 552
parameters 548
SLOPETOL option
simulation time 337
timestep control 335
SMOOTH element parameter 191
SONAME model parameter 204
source
data driven 142
keywords 120
statements 41
See also independent sources
SOVHI model parameter 204
SOVLO model parameter 204
.sp file 611, 613
SPICE
compatibility
AC output 262–263
plot 245
sqrt(x) function 229
square root function 229
.st# file 16, 19
634
starting
hspice 20
hspicerf 22
interactively 23
statement
.DOUT 213
statements
.AC 547
.DATA 50
.DC 295, 469, 547
.DCVOLT 293
DOUT 242
element 41
.ENDL 51
.GRAPH 242, 245, 249
.IC 293
initial conditions 293
.LIB 51
.LOAD 294, 295
.MEASURE 242, 243, 267
.MODEL 547
.OP 291
.OPTION
CO 248, 249
.PARAM 52
.PLOT 242, 244, 249
.PRINT 242, 243, 249
.PROBE 242, 245, 249
.SAVE 294
source 41
.STIM 242, 274
.SUBCKT 269
.TEMP 50, 547, 548
.TRAN 547
statistical analysis 548–577
statistics
calculations 545
.STIM statement 242, 274
stimuli 274
structure simulation 5
subcircuit cross-listing file 19
subcircuits
adder 507
calling tree 48
changing in .ALTER blocks 53
creating reusable circuits 57
hierarchical parameters 58
library structure 63
Index
T
multiplying 58
node names 47, 48
output printing 249
path names 48
power dissipation computation 256
.PRINT and .PLOT statements 60
search order 60
zero prefix 49
.SUBCKT statement 269
.sw# file 15, 17
sweep
variables 519
switch example 192
switch-level MOSFET’s example 192
T
tabular data 211
Taguchi analysis 544
tan(x) function 229
tanh(x) function 229
TC1, TC2 element parameters 175
TD parameter 175, 182, 192, 197, 264, 270
TDELAY statement 216
TEMP
directory 21
environment variable 21
model parameter 50, 547
sweep variable 519
.TEMP statement 547, 548
temper variable 233
temperature
circuit 545, 547
coefficients 66, 518
derating 50, 547
element 547
optimizing coefficients 519
reference 50, 547
sweeping 519
variable 233
Temperature Variation Analysis 544
.TF statement 296
three-dimensional function 160
TIC model parameter 246
time
delay 264
domain algorithm 331
variable 232
TIMESCALE model parameter 204
timestep
algorithms 334
control
algorithms 333–336
CHGTOL 335
DELMAX 336
FS 336
FT 336
minimum internal timestep 336
Minimum Timestep Coefficient 336
options 328, 335
RELQ 335
RMAX 336
RMIN 336
TRTOL 335
TSTEP 336
default control algorithm 330
DVDT algorithm 335
local truncation error algorithm 334
reversal 334
TIMESTEP model parameter 204
title for simulation 40
.TITLE statement 40
TMP directory 21
tmp directory 21
TMP environment variable 21
tmpdir environment variable 21
TNOM option 50, 547
TOX model parameter 549
.tr# file 16, 19
.TRAN statement 469, 547
transconductance
FREQ function 169
LAPLACE function 167
POLE function 168
transfer sign function 230
transient
analysis 243
initial conditions 293, 316
inverter 320
RC network 318
sources 124
output variables 251
transient analysis measurement results file 19
transient analysis results file 19
transmission lines
example 513
635
Index
U
U Element 109
trapezoidal integration
algorithm 330
TREF model parameter 547, 548
triode tube 194
TRTOL option 335
truncation algorithm 334
TSTEP
timestep control 336
two-dimensional function 159
U
U Elements 199
digital input 199
UIC
analysis parameter 291
transient analysis parameter 317
UNIF keyword 557
uniform parameter distribution 553
unity gain frequency 520
UTRA model parameter restriction 304
V
variability
defined in HSPICE 431
introduction 431
simulating 431
variation block 432
variable, environment, METAHOME 613
variables
AC formats 263
changing in .ALTER blocks 53
DEFAULT_INCLUDE 14
Hspice-specific 232
output 243
AC 260
DC 251
transient 251
plotting 509
sweeping 519
TEMP 21
TMP 21
tmpdir 21
variables, environment 11
variance, statistical 545
variation block
absolute vs relative variation 442
access functions 442
advantages 432
dependent random variables 437
element parameter variations 439
example 443
general section 434
options 435
global sub-blocks 435
independent random variables 436
local sub-blocks 435
model parameter variations 438
overview 433
structure 434
variation block options
Monte Carlo 450
VCCAP 188
VCCS See voltage controlled current source
VCR See voltage controlled resistor
VCVS See voltage controlled voltage source
vector patterns 211
vendor libraries 62
Verilog value format 214
version
95.3 compatibility 336
VIH statement 217
VIL statement 217
Vnn node name in CSOS 49
VOH statement 217
VOL keyword 177
voltage
failure 308
gain
FREQ function 169
LAPLACE function 167
POLE function 168
initial conditions 293
logic high 217
217
nodal output DC 252
sources 165, 195, 252
summer
636
logicw
Index
W
VREF statement 217
VTH statement 217
Vxxx source element statement 120
W
W Elements 101
warnings
all nodes connected together 306
floating power supply nodes 48
zero diagonal value detected 307
waveform
characteristics 216
Waveform Characteristics section 216
WHEN keyword 270, 520
.WIDTH
for printout width 248
wildcard uses 45
WMAX model parameter 5
WMIN model parameter 5
worst case analysis 548, 568, 577
Worst Case Corners Analysis 544
XL model parameter 549
XMAX model parameter 246
XMIN model parameter 246
XPHOTO model parameter 565
XSCAL model parameter 246
XW model parameter 549
Y
YGRID model parameter 246
yield analysis 544
YIN keyword 265, 387
YMAX parameter 247
YMIN parameter 247
YOUT keyword 265, 387
YSCAL model parameter 247
Z
zero delay gate 177, 193
ZIN keyword 265, 387
ZOUT keyword 265, 387
X
XGRID model parameter 246
637
Index
Z
638
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