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

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

Download PDF

advertisement