HSPICE® Simulation and Analysis User Guide Version X-2005.09, September 2005 Copyright Notice and Proprietary Information Copyright 2005 Synopsys, Inc. All rights reserved. This software and documentation contain confidential and proprietary information that is the property of Synopsys, Inc. The software and documentation are furnished under a license agreement and may be used or copied only in accordance with the terms of the license agreement. No part of the software and documentation may be reproduced, transmitted, or translated, in any form or by any means, electronic, mechanical, manual, optical, or otherwise, without prior written permission of Synopsys, Inc., or as expressly provided by the license agreement. Right to Copy Documentation The license agreement with Synopsys permits licensee to make copies of the documentation for its internal use only. Each copy shall include all copyrights, trademarks, service marks, and proprietary rights notices, if any. Licensee must assign sequential numbers to all copies. These copies shall contain the following legend on the cover page: “This document is duplicated with the permission of Synopsys, Inc., for the exclusive use of __________________________________________ and its employees. This is copy number __________.” Destination Control Statement All technical data contained in this publication is subject to the export control laws of the United States of America. Disclosure to nationals of other countries contrary to United States law is prohibited. It is the reader’s responsibility to determine the applicable regulations and to comply with them. Disclaimer SYNOPSYS, INC., AND ITS LICENSORS MAKE NO WARRANTY OF ANY KIND, EXPRESS OR IMPLIED, WITH REGARD TO THIS MATERIAL, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE. Registered Trademarks (®) Synopsys, AMPS, Arcadia, C Level Design, C2HDL, C2V, C2VHDL, Cadabra, Calaveras Algorithm, CATS, CRITIC, CSim, Design Compiler, DesignPower, DesignWare, EPIC, Formality, HSIM, HSPICE, Hypermodel, iN-Phase, in-Sync, Leda, MAST, Meta, Meta-Software, ModelTools, NanoSim, OpenVera, PathMill, Photolynx, Physical Compiler, PowerMill, PrimeTime, RailMill, RapidScript, Saber, SiVL, SNUG, SolvNet, Superlog, System Compiler, Testify, TetraMAX, TimeMill, TMA, VCS, Vera, and Virtual Stepper are registered trademarks of Synopsys, Inc. Trademarks (™) Active Parasitics, AFGen, Apollo, Apollo II, Apollo-DPII, Apollo-GA, ApolloGAII, Astro, Astro-Rail, Astro-Xtalk, Aurora, AvanTestchip, AvanWaves, BCView, Behavioral Compiler, BOA, BRT, Cedar, ChipPlanner, Circuit Analysis, Columbia, Columbia-CE, Comet 3D, Cosmos, CosmosEnterprise, CosmosLE, CosmosScope, CosmosSE, Cyclelink, Davinci, DC Expert, DC Expert Plus, DC Professional, DC Ultra, DC Ultra Plus, Design Advisor, Design Analyzer, Design Vision, DesignerHDL, DesignTime, DFM-Workbench, Direct RTL, Direct Silicon Access, Discovery, DW8051, DWPCI, Dynamic-Macromodeling, Dynamic Model Switcher, ECL Compiler, ECO Compiler, EDAnavigator, Encore, Encore PQ, Evaccess, ExpressModel, Floorplan Manager, Formal Model Checker, FoundryModel, FPGA Compiler II, FPGA Express, Frame Compiler, Galaxy, Gatran, HANEX, HDL Advisor, HDL Compiler, Hercules, Hercules-Explorer, Hercules-II, Hierarchical Optimization Technology, High Performance Option, HotPlace, HSIMplus, HSPICE-Link, iN-Tandem, Integrator, Interactive Waveform Viewer, i-Virtual Stepper, Jupiter, Jupiter-DP, JupiterXT, JupiterXT-ASIC, JVXtreme, Liberty, Libra-Passport, Library Compiler, Libra-Visa, Magellan, Mars, Mars-Rail, Mars-Xtalk, Medici, Metacapture, Metacircuit, Metamanager, Metamixsim, Milkyway, ModelSource, Module Compiler, MS-3200, MS-3400, Nova Product Family, Nova-ExploreRTL, Nova-Trans, Nova-VeriLint, Nova-VHDLlint, Optimum Silicon, Orion_ec, Parasitic View, Passport, Planet, Planet-PL, Planet-RTL, Polaris, Polaris-CBS, Polaris-MT, Power Compiler, PowerCODE, PowerGate, ProFPGA, ProGen, Prospector, Protocol Compiler, PSMGen, Raphael, Raphael-NES, RoadRunner, RTL Analyzer, Saturn, ScanBand, Schematic Compiler, Scirocco, Scirocco-i, Shadow Debugger, Silicon Blueprint, Silicon Early Access, SinglePass-SoC, Smart Extraction, SmartLicense, SmartModel Library, Softwire, Source-Level Design, Star, Star-DC, Star-MS, Star-MTB, Star-Power, Star-Rail, Star-RC, Star-RCXT, Star-Sim, Star-SimXT, Star-Time, Star-XP, SWIFT, Taurus, TimeSlice, TimeTracker, Timing Annotator, TopoPlace, TopoRoute, Trace-On-Demand, True-Hspice, TSUPREM-4, TymeWare, VCS Express, VCSi, Venus, Verification Portal, VFormal, VHDL Compiler, VHDL System Simulator, VirSim, and VMC are trademarks of Synopsys, Inc. Service Marks (SM) MAP-in, SVP Café, and TAP-in are service marks of Synopsys, Inc. SystemC is a trademark of the Open SystemC Initiative and is used under license. ARM and AMBA are registered trademarks of ARM Limited. All other product or company names may be trademarks of their respective owners. Printed in the U.S.A. HSPICE® Simulation and Analysis User Guide, X-2005.09 ii HSPICE® Simulation and Analysis User Guide X-2005.09 Contents About This Manual xxiii Inside This Manual. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxiii The HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxv Searching Across the HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . xxvi Other Related Publications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxvi Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxvii Customer Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xxviii Accessing SolvNet xxviii Contacting the Synopsys Technical Support Center xxviii 1. 2. Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 HSPICE Varieties. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 HSPICE Features for Running Higher-Level Simulations . . . . . . . . . . . . 5 Simulation Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6 Experimental Methods Supported by HSPICE . . . . . . . . . . . . . . . . . . . . 6 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 HSPICE® Simulation and Analysis User Guide X-2005.09 iii Contents iv DC Operating Point Initial Conditions File). . . . . . . . . . . . . . . . . . . . . . . . 15 Input Netlist File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15 Library Input File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15 Analog Transition Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15 Standard Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16 AC Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 AC Analysis Measurement Reults File . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 DC Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 DC Analysis Measurement Results File. . . . . . . . . . . . . . . . . . . . . . . . . . 18 Digital Output File. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 FFT Analysis Graph Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Hardcopy Graph Data File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 HBLSP Analysis Extraction Results File . . . . . . . . . . . . . . . . . . . . . . . . . 18 HBLSP Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 HBLSP Analysis Print Information File. . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Operating Point Information File. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Operating Point Node Voltages File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Output Listing File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Output Status File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 Output Tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21 Subcircuit Cross-Listing File. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21 Transient Analysis Measurement Results File . . . . . . . . . . . . . . . . . . . . . 21 Transient Analysis Results File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21 Starting HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22 Redirecting Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 23 Running an HSPICE Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24 Interactive Simulation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Examples of Starting HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Starting HSPICE RF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28 Improving Simulation Performance with Multithreading . . . . . . . . . . . . . . . . . . 29 Running HSPICE-MT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29 Performance Improvement Estimations . . . . . . . . . . . . . . . . . . . . . . . . . . 30 Simulating in Client/Server Mode. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30 Server. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Client . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Simulating with Stand-alone .MEASURE Calculations . . . . . . . . . . . . . . . . . . 33 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents 3. Input Netlist and Data Entry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Input Netlist File Guidelines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Input Line Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . First Character . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 38 Delimiters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38 Node Identifiers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 Instance Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 Hierarchy Paths . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41 Numbers. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41 Parameters and Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 Input Netlist File Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 Schematic Netlists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 Input Netlist File Composition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Title of Simulation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 Comments and Line Continuation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Element and Source Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48 Defining Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 Node Naming Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Using Wildcards on Node Names . . . . . . . . . . . . . . . . . . . . . . . . . . 50 51 Element, Instance, and Subcircuit Naming Conventions . . . . . . . . . . . . . 53 Subcircuit Node Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53 Path Names of Subcircuit Nodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54 Abbreviated Subcircuit Node Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Automatic Node Name Generation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Global Node Names. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56 Circuit Temperature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56 Data-Driven Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56 Library Calls and Definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Library Building Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 57 Automatic Library Selection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 Defining Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Predefined Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Measurement Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58 58 59 Altering Design Variables and Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . Using Multiple .ALTER Blocks . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59 60 Connecting Nodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60 Deleting a Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61 Ending a Netlist . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61 HSPICE® Simulation and Analysis User Guide X-2005.09 v Contents 4. vi Condition-Controlled Netlists (IF-ELSE). . . . . . . . . . . . . . . . . . . . . . . . . . 61 Using Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63 Hierarchical Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . M (Multiply) Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . S (Scale) Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Using Hierarchical Parameters to Simplify Simulation . . . . . . . . . . . 64 64 65 65 Undefined Subcircuit Search . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66 Subcircuit Call Statement Discrete Device Libraries. . . . . . . . . . . . . . . . . . . . 67 DDL Library Access . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67 Vendor Libraries . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68 Subcircuit Library Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69 Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 Passive Elements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 Values for Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 Resistor Elements in a HSPICE or HSPICE RF Netlist . . . . . . . . . . . . . . Linear Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Behavioral Resistors in HSPICE or HSPICE RF . . . . . . . . . . . . . . . Frequency-Dependent Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . . Skin Effect Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 72 74 75 76 77 Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Linear Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Frequency-Dependent Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . Behavioral Capacitors in HSPICE or HSPICE RF . . . . . . . . . . . . . . DC Block Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Charge-Conserved Capacitors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 77 80 81 83 83 84 Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Mutual Inductors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Ideal Transformer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Linear Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Frequency-Dependent Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . AC Choke Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85 88 90 92 93 94 Active Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Diode Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Bipolar Junction Transistor (BJT) Element . . . . . . . . . . . . . . . . . . . . . . . . 97 JFETs and MESFETs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100 MOSFETs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102 Transmission Lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105 W Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents 5. W Element Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106 Lossless (T Element) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Ideal Transmission Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110 112 Lossy (U Element) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 114 Frequency-Dependent Multi-Terminal S Element . . . . . . . . . . . . . . . . . . 115 Frequency Table Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121 Group Delay Handler in Time Domain Analysis . . . . . . . . . . . . . . . . . . . . 121 Pre-Conditioning S Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 122 IBIS Buffers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 Sources and Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125 Independent Source Elements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125 Source Element Conventions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 Independent Source Element. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 DC Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129 AC Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130 Transient Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130 Mixed Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130 Port Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 131 Independent Source Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135 Pulse Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135 Sinusoidal Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Exponential Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 142 Piecewise Linear (PWL) Source Function . . . . . . . . . . . . . . . . . . . . . . . . General Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . MSINC and ASPEC Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145 145 145 Data-Driven Piecewise Linear Source . . . . . . . . . . . . . . . . . . . . . . . . . . . 147 Single-Frequency FM Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . 149 Amplitude Modulation Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . 151 Pattern Source Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Nested-Structure Pattern Source . . . . . . . . . . . . . . . . . . . . . . . . . . . Pattern-Command Driven Pattern Source . . . . . . . . . . . . . . . . . . . . 153 156 157 Pseudo Random-Bit Generator Source (PRBS Function) . . . . . . . . . . . . Linear Feedback Shift Register . . . . . . . . . . . . . . . . . . . . . . . . . . . . Conventions for Feedback Tap Specification . . . . . . . . . . . . . . . . . . PRBS Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 158 159 159 160 Voltage and Current Controlled Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162 Polynomial Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164 HSPICE® Simulation and Analysis User Guide X-2005.09 vii Contents viii One-Dimensional Function. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Two-Dimensional Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Three-Dimensional Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164 165 166 Piecewise Linear Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167 Power Sources. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168 Independent Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Outputs. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168 171 Controlled Sources. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 171 Voltage-Dependent Voltage Sources — E Elements . . . . . . . . . . . . . . . . . . . . 171 Voltage-Controlled Voltage Source (VCVS) . . . . . . . . . . . . . . . . . . . . . . . Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Multi-Input Gates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Laplace Transform . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Pole-Zero Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Frequency Response Table . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 172 172 172 172 172 172 173 174 175 Behavioral Voltage Source . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 176 Ideal Op-Amp . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 176 Ideal Transformer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 176 E Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Ideal OpAmp . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Voltage Summer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Polynomial Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Zero-Delay Inverter Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Ideal Transformer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Voltage-Controlled Oscillator (VCO). . . . . . . . . . . . . . . . . . . . . . . . . 179 179 180 180 181 181 181 Using the E Element for AC Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . 181 Current-Dependent Current Sources — F Elements . . . . . . . . . . . . . . . . . . . . 182 Current-Controlled Current Source (CCCS) Syntax. . . . . . . . . . . . . . . . . Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Multi-Input Gates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 182 182 182 183 183 183 Voltage-Dependent Current Sources — G Elements. . . . . . . . . . . . . . . . . . . . 186 Voltage-Controlled Current Source (VCCS) . . . . . . . . . . . . . . . . . . . . . . . Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186 187 187 187 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents Multi-Input Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Laplace Transform . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Pole-Zero Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Frequency Response Table . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187 187 187 188 188 Behavioral Current Source (Noise Model) Syntax . . . . . . . . . . . . . . . . . . 188 Voltage-Controlled Resistor (VCR) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Multi-Input Gates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 188 188 189 189 189 Voltage-Controlled Capacitor (VCCAP) . . . . . . . . . . . . . . . . . . . . . . . . . . NPWL Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . PPWL Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 189 190 190 G Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Switch. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Switch-Level MOSFET . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Voltage-Controlled Capacitor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Zero-Delay Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Diode Equation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Diode Breakdown . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Triodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Behavioral Noise Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 193 193 193 193 194 194 194 194 195 195 Current-Dependent Voltage Sources — H Elements. . . . . . . . . . . . . . . . . . . . 195 Current-Controlled Voltage Source (CCVS) . . . . . . . . . . . . . . . . . . . . . . . Linear . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Polynomial (POLY) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Piecewise Linear (PWL) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Multi-Input Gate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Delay Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 195 195 196 196 196 196 H Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 198 Digital and Mixed Mode Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199 U Element Digital Input Elements and Models. . . . . . . . . . . . . . . . . . . . . General Form . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Model Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Digital-to-Analog Input Model Parameters . . . . . . . . . . . . . . . . . . . . 199 200 201 201 U Element Digital Outputs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Model Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Analog-to-Digital Output Model Parameters. . . . . . . . . . . . . . . . . . . 203 203 204 Replacing Sources With Digital Inputs. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 206 Specifying a Digital Vector File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 208 HSPICE® Simulation and Analysis User Guide X-2005.09 ix Contents Commands in a Digital Vector File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6. x 209 Vector Patterns. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 209 Defining Tabular Data. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Input Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Expected Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Verilog Value Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Periodic Tabular Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 209 210 211 212 213 Waveform Characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214 Modifying Waveform Characteristics . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214 Using the Context-Based Control Option . . . . . . . . . . . . . . . . . . . . . . . . . 215 Comment Lines and Line Continuations . . . . . . . . . . . . . . . . . . . . . . . . . 216 Parameter Usage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . First Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Second Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Third Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 216 216 217 217 Digital Vector File Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 218 Parameters and Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 221 Using Parameters in Simulation (.PARAM) . . . . . . . . . . . . . . . . . . . . . . . . . . . 222 Defining Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 222 Assigning Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Inline Parameter Assignments . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Parameters in Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 224 224 224 User-Defined Function Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 225 Predefined Analysis Function. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 225 Measurement Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 225 .PRINT|.PROBE|.PLOT|.GRAPH Parameters . . . . . . . . . . . . . . . . . . . . . 226 Multiply Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 226 Using Algebraic Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 226 Built-In Functions and Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 227 Parameter Scoping and Passing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 232 Library Integrity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233 Reusing Cells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233 Creating Parameters in a Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233 String Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 236 Parameter Defaults and Inheritance. . . . . . . . . . . . . . . . . . . . . . . . . . . . . Parameter Passing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 237 238 Parameter Passing Solutions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 240 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents 7. Simulation Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241 Overview of Output Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241 Output Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241 Output Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 243 Displaying Simulation Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 244 .PRINT Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Statement Order. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 244 244 .PLOT Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 245 .PROBE Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 245 .GRAPH Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .MODEL Statement for .GRAPH . . . . . . . . . . . . . . . . . . . . . . . . . . . 246 246 Using Wildcards in PRINT, PROBE, PLOT, and GRAPH Statements . . . Supported Wildcard Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . 247 248 Print Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Changing the File Descriptor Limit . . . . . . . . . . . . . . . . . . . . . . . . . . 249 249 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 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 251 252 252 252 253 256 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. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 260 261 262 263 264 264 265 265 266 Element Template Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 267 Specifying User-Defined Analysis (.MEASURE) . . . . . . . . . . . . . . . . . . . . . . . 268 .MEASURE Statement Order. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269 .MEASURE Parameter Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269 FIND and WHEN Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271 Equation Evaluation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271 Average, RMS, MIN, MAX, INTEG, and PP . . . . . . . . . . . . . . . . . . . . . . . 271 HSPICE® Simulation and Analysis User Guide X-2005.09 xi Contents xii INTEGRAL Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 272 DERIVATIVE Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 272 ERROR Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Error Equations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 272 273 .SURGE Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274 .CHECK Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 275 Setting Global Hi/Lo Levels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 275 Slew, Rise, and Fall Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 276 Edge Timing Verification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 278 Setup and Hold Verification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 279 IR Drop Detection. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 281 DSPF Flow. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 282 How HSPICE RF Uses a DSPF File . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284 SIM_DSPF_SCALER/SIM_DSPF_SCALEC . . . . . . . . . . . . . . . . . . . . . . 284 Selective DSPF Expansion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 285 Multi-Threshold Selective DSPF Expansion . . . . . . . . . . . . . . . . . . . . . . 286 Sample DSPF Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 287 Reusing Simulation Output as Input Stimuli. . . . . . . . . . . . . . . . . . . . . . . . . . . 287 Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 288 .POWER Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 289 SIM_POWERSTART and SIM_POWERSTOP Options . . . . . . . . . . . . . . 290 SIM_POWERPOST Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 290 POWER_TOP Option. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 290 POWER_ANALYSIS Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 291 Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 292 .POWERDC Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 294 Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 295 Element Template Listings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 296 Analog Compression . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . SIM_DELTAV (Voltage). . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . SIM_DELTAI (Current) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 308 308 309 Tabulated Data Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 309 WDB Output Format. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 310 XP Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 310 NW Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 310 VCD Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 Turbowave Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 Undertow Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents Limiting Output Data Size in HSPICE RF . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8. 311 SIM_POSTTOP Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 312 SIM_POSTSKIP Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 312 SIM_POSTAT Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 312 SIM_POSTDOWN Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 313 SIM_POSTSCOPE Option. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 313 Node Hierarchy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 314 Initializing DC/Operating Point Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 315 Simulation Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 315 Initialization and Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 316 DC Initialization and Operating Point Calculation . . . . . . . . . . . . . . . . . . . . . . 319 .OP Statement — Operating Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319 319 Element Statement IC Parameter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 320 Initial Conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 321 SAVE and LOAD Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .SAVE Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .LOAD Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 321 322 323 .DC Statement—DC Sweeps. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 323 Other DC Analysis Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324 DC Initialization Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324 Accuracy and Convergence . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 325 Accuracy Tolerances . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 325 Accuracy Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328 Autoconverge Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . DCON and GMINDC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328 330 Reducing DC Errors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 332 Shorted Element Nodes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 334 Inserting Conductance, Using DCSTEP . . . . . . . . . . . . . . . . . . . . . . . . . 334 Floating-Point Overflow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 335 Diagnosing Convergence Problems. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 335 Non-Convergence Diagnostic Table. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 336 Traceback of Non-Convergence Source . . . . . . . . . . . . . . . . . . . . . . . . . 337 Solutions for Non-Convergent Circuits . . . . . . . . . . . . . . . . . . . . . . . . . . . Poor Initial Conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 338 338 HSPICE® Simulation and Analysis User Guide X-2005.09 xiii Contents 9. xiv Inappropriate Model Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . PN Junctions (Diodes, MOSFETs, BJTs). . . . . . . . . . . . . . . . . . . . . 339 341 Transient Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 343 Simulation Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 343 Overview of Transient Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 344 Transient Analysis Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 346 Transient Analysis of an RC Network. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 347 Transient Analysis of an Inverter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 348 Using the .BIASCHK Statement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 350 Data Checking Methods. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Limit and Noise Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Maximum Method. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Minimum Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Region Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 351 351 352 352 352 Transient Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 353 Matrix Manipulation Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 353 Simulation Speed and Accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Simulation Speed . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Simulation Accuracy. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Timestep Control for Accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Models and Accuracy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Guidelines for Choosing Accuracy Options . . . . . . . . . . . . . . . . . . . 355 355 356 357 Linear Acceleration (SIM_LA Option) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 357 PACT Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 358 PI Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Specifying Maximum Resistance . . . . . . . . . . . . . . . . . . . . . . . . . . . Specifying Minimum Capacitance . . . . . . . . . . . . . . . . . . . . . . . . . . 359 360 360 Other PACT Options (HSPICE RF) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Specifying Error Tolerance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Specifying Upper Frequency . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Specifying Minimum Switching Time . . . . . . . . . . . . . . . . . . . . . . . . Node Reduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 360 360 361 361 362 SIM_LA Options Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 362 Numerical Integration Algorithm Controls (HSPICE) . . . . . . . . . . . . . . . . . . . . 363 Gear and Trapezoidal Algorithms. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 363 Numerical Integration Algorithm Controls (HSPICE RF) . . . . . . . . . . . . . . . . . 366 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents Selecting Timestep Control Algorithms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 366 Iteration Count Dynamic Timestep Algorithm. . . . . . . . . . . . . . . . . . . . . . 368 Local Truncation Error (LTE) Dynamic Timestep . . . . . . . . . . . . . . . . . . . 368 DVDT Dynamic Timestep Algorithm. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 368 Timestep Controls in HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 370 Timestep Control in HSPICE RF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION SIM_ACCURACY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION METHOD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION MAXORD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION SIM_ORDER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION SIM_TG_THETA. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION SIM_TRAP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION PURETP . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .OPTION SIM_OSC_DETECT_TOL . . . . . . . . . . . . . . . . . . . . . . . . Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 371 371 372 373 373 373 373 373 373 374 Fourier Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Accuracy and DELMAX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Fourier Equation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 375 376 376 10. AC Sweep and Small Signal Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 379 Using the .AC Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 379 .AC Control Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 380 AC Small Signal Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 380 AC Analysis of an RC Network . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 382 Other AC Analysis Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 385 Using .DISTO for Small-Signal Distortion Analysis . . . . . . . . . . . . . . . . . 385 Using .NOISE for Small-Signal Noise Analysis . . . . . . . . . . . . . . . . . . . . 385 Using .SAMPLE for Noise Folding Analysis . . . . . . . . . . . . . . . . . . . . . . . 387 11. Linear Network Parameter Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 389 .LIN Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 389 Identifying Ports with the Port Element . . . . . . . . . . . . . . . . . . . . . . . . . . 390 Using the P (Port) Element for Mixed-Mode Measurement . . . . . . . . . . . 394 .LIN Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 .LIN Output Syntax. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . PARAM Definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . TYPE Definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 396 398 Multi-Port Scattering (S) Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . 398 HSPICE® Simulation and Analysis User Guide X-2005.09 xv Contents xvi 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 . . . . . . . 399 400 400 400 401 401 401 402 402 Noise Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 403 Hybrid (H) Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 Group Delay . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 RF Measurements From .LIN . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 405 Impedance Characterizations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406 Stability Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406 Gain Measurements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406 Matching for Optimal Gain . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 406 Noise Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 407 Two-Port Transfer and Noise Measurements . . . . . . . . . . . . . . . . . . . . . . 407 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. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 408 408 408 409 409 409 409 410 410 411 411 412 413 413 413 414 415 Extracting Mixed-Mode Scattering (S) Parameters . . . . . . . . . . . . . . . . . . . . . 415 Defaults . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 416 Output File Formats . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 417 Two-Port Parameter Measurement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 417 Output Format and Description . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 418 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents Features Supported . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 419 Prerequisites and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 419 Reported Statistics for the Performance Log (HSPICE RF Only) . . . . . . 419 Errors and Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 420 .NET Parameter Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 420 Network Analysis Example: Bipolar Transistor. . . . . . . . . . . . . . . . . . . . . 423 .NET Parameter Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 424 Bandpass Netlist: Network Analysis Results . . . . . . . . . . . . . . . . . . . . . . 425 References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 426 12. Using HSPICE with Verilog-A . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 429 Getting Started. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 430 Example: JFET Compact Device Model . . . . . . . . . . . . . . . . . . . . . . . . . 430 Introduction to Verilog-A. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 433 Verilog-A Module Template . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 433 Data Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 434 Analog Operators and Filters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 434 Mathematical Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 436 Transcendental Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 437 AC Analysis Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 438 Noise Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 439 Analog Events . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 439 Timestep and Simulator Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 440 System Tasks and I/O Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 441 Simulator Environment Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 442 Module Hierarchy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 442 Simulation with Verilog-A Modules. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 443 Loading Verilog-A Devices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 443 HSPICE .hdl Netlist Command . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 444 HSPICE -hdl Command-line Option. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 444 Verilog-A Search Path . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 444 HSPICE -vamodel Command-line Option . . . . . . . . . . . . . . . . . . . . . . . . 445 Verilog-A File Loading Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . 446 Verilog-A Behavior in a .ALTER Analysis . . . . . . . . . . . . . . . . . . . . . . . . . 446 Instantiating Verilog-A Devices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 447 Using Model Cards with Verilog-A Modules . . . . . . . . . . . . . . . . . . . . . . . 448 HSPICE® Simulation and Analysis User Guide X-2005.09 xvii Contents xviii Restrictions on Verilog-A Module Names. . . . . . . . . . . . . . . . . . . . . . . . . 449 Overriding Subcircuits with Verilog-A Modules . . . . . . . . . . . . . . . . . . . . Netlist Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Command-line Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 450 450 451 Disabling .OPTION vamodel with .OPTION spmodel . . . . . . . . . . . . . . . 452 Using Vector Buses or "Ports" . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 453 Using Integer Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 453 Implicit Parameter M Support. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 453 Module and Parameter Name Case Sensitivity . . . . . . . . . . . . . . . . . . . . . . . . 454 Module Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 454 Module Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 454 Output Simulation Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 455 V() and I() Access Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 455 Output Bus Signals . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 456 Output Internal Module Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 457 Output Module Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 458 Verilog-A Device Output Simulation Data. . . . . . . . . . . . . . . . . . . . . . . . . 458 Using Wildcards in Verilog-A . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 459 Port Probing and Branch Current Reporting Conventions . . . . . . . . . . . . 460 Unsupported Output Function Features. . . . . . . . . . . . . . . . . . . . . . . . . . 460 Using the Stand-alone Compiler . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 460 Setting Environment Option for HSPICE Verilog-A Compiler. . . . . . . . . . . . . . 461 The Compiled Model Library Cache . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 461 Cache Location . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 462 Deleting the Cache. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 462 Unsupported Language Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 463 Known Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 467 analysis() Function Behavior . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 467 13. DC Mismatch Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 469 Mismatch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 469 Simulation Methods for Variability . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 469 DCmatch Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 470 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 471 DCmatch Definition Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 472 472 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents Accessing Instance Parameters in Expressions for Sigma . . . . . . . 473 DCmatch Table Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 473 Output From .PROBE and .MEASURE Commands . . . . . . . . . . . . . . . . Syntax for .PROBE Command . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Syntax for .MEASURE Command . . . . . . . . . . . . . . . . . . . . . . . . . . 475 475 475 Practical Considerations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . DCmatch Variability as a Function of Device Geometry. . . . . . . . . . Parameter Traceability . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 476 476 477 Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 477 Reference List . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 478 14. Statistical Analysis and Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 479 Analytical Model Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 480 Simulating Circuit and Model Temperatures . . . . . . . . . . . . . . . . . . . . . . . . . . 481 Temperature Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 483 .TEMP Statement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 484 Worst Case Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 484 Model Skew Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Using Skew Parameters in HSPICE . . . . . . . . . . . . . . . . . . . . . . . . . Skew File Interface to Device Models. . . . . . . . . . . . . . . . . . . . . . . . 484 486 488 Monte Carlo Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 489 Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Gaussian Parameter Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . Uniform Parameter Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . . Random Limit Parameter Distribution. . . . . . . . . . . . . . . . . . . . . . . . 489 489 489 490 Monte Carlo Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 490 Monte Carlo Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 492 .PARAM Distribution Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 492 Monte Carlo Parameter Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 494 Monte Carlo Examples. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Gaussian, Uniform, and Limit Functions . . . . . . . . . . . . . . . . . . . . . Major and Minor Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . RC Time Constant . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Switched Capacitor Filter Design . . . . . . . . . . . . . . . . . . . . . . . . . . . 495 495 497 498 499 Worst Case and Monte Carlo Sweep Example . . . . . . . . . . . . . . . . . . . . . . . . 502 HSPICE Input File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 502 Transient Sigma Sweep Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 503 Monte Carlo Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 504 HSPICE® Simulation and Analysis User Guide X-2005.09 xix Contents Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xx 510 Optimization Control. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 511 Simulation Accuracy. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 512 Curve Fit Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 512 Goal Optimization. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 513 Timing Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 513 Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Optimizing Analysis (.DC, .TRAN, .AC) . . . . . . . . . . . . . . . . . . . . . . 514 515 Optimization Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 515 MOS Level 3 Model DC Optimization. . . . . . . . . . . . . . . . . . . . . . . . . . . . Input Netlist File for Level 3 Model DC Optimization . . . . . . . . . . . . 516 516 MOS Level 13 Model DC Optimization. . . . . . . . . . . . . . . . . . . . . . . . . . . DC Optimization Input Netlist File for Level 13 Model . . . . . . . . . . . 518 519 RC Network Optimization. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Optimization Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Optimized Parameters OPTRC . . . . . . . . . . . . . . . . . . . . . . . . . . . . 520 520 522 Optimizing CMOS Tristate Buffer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Input Netlist File to Optimize a CMOS Tristate Buffer. . . . . . . . . . . . 523 524 BJT S Parameters Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Key HSPICE Features Used . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Input Netlist File for Optimizing BJT S Parameters . . . . . . . . . . . . . 525 526 526 BJT Model DC Optimization. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . BJT Model DC Optimization Input Netlist File . . . . . . . . . . . . . . . . . 527 528 Optimizing GaAsFET Model DC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . GaAsFET Model DC Optimization Input Netlist File. . . . . . . . . . . . . 529 530 Optimizing MOS Op-amp . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . MOS Op-amp Optimization Input Netlist File . . . . . . . . . . . . . . . . . . 530 531 15. Running Demonstration Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 533 Using the Demo Directory Tree . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 534 Two-Bit Adder Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 535 One-Bit Subcircuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 535 MOS Two-Bit Adder Input File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 536 MOS I-V and C-V Plotting Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 536 Plotting Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 537 MOS I-V and C-V Plot Example Input File . . . . . . . . . . . . . . . . . . . . . . . . 541 CMOS Output Driver Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 541 Strategy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 542 HSPICE® Simulation and Analysis User Guide X-2005.09 Contents CMOS Output Driver Example Input File . . . . . . . . . . . . . . . . . . . . . . . . . A. 546 Temperature Coefficients Demo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 546 Input File for Optimized Temperature Coefficients . . . . . . . . . . . . . . . . . . 547 Optimization Section . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 548 Simulating Electrical Measurements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 548 T2N2222 Optimization Example Input File. . . . . . . . . . . . . . . . . . . . . . . . 549 Modeling Wide-Channel MOS Transistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . 549 Demonstration Input Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 552 Full Simulation Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 571 Simulation Example Using AvanWaves . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 571 Input Netlist and Circuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 571 Execution and Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Example.ic . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Example.lis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Example.st0 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 573 574 574 577 Simulation Graphical Output in AvanWaves. . . . . . . . . . . . . . . . . . . . . . . 580 Simulation Example Using Cosmos-Scope . . . . . . . . . . . . . . . . . . . . . . . . . . . 587 Input Netlist and Circuit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 587 Execution and Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 589 View HSPICE Results in Cosmos-Scope. . . . . . . . . . . . . . . . . . . . . . . . . Viewing HSPICE Transient Analysis Waveforms . . . . . . . . . . . . . . . Viewing HSPICE AC Analysis Waveforms . . . . . . . . . . . . . . . . . . . . Viewing HSPICE DC Analysis Waveforms . . . . . . . . . . . . . . . . . . . . 590 590 592 594 Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 597 HSPICE® Simulation and Analysis User Guide X-2005.09 xxi Contents xxii HSPICE® Simulation and Analysis User Guide X-2005.09 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. HSPICE® Simulation and Analysis User Guide X-2005.06 xxiii About This Manual Inside This Manual xxiv Chapter Description 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. 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 HSPICE with Verilog-A Describes how to use Verilog-A in HSPICE simulations. Chapter 13, DC Mismatch Analysis Describes the use of DCmatch analysis. Chapter 14, Statistical Analysis and Optimization Describes how to use statistical analysis and optimization in HSPICE to analyze and optimize electrical yield. Chapter 15, 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, Full Simulation Examples Contains information and sample input netlists for two full simulation examples. HSPICE® Simulation and Analysis User Guide X-2005.06 About This Manual The HSPICE Documentation Set The HSPICE Documentation Set This manual is a part of the HSPICE documentation set, which includes the following manuals: Manual Description HSPICE Simulation and Analysis User Guide Describes how to use HSPICE to simulate and analyze your circuit designs. This is the main HSPICE user guide. HSPICE Signal Integrity Guide Describes how to use HSPICE to maintain signal integrity in your chip design. HSPICE Applications Manual Provides application examples and additional HSPICE user information. HSPICE Command Reference Provides reference information for HSPICE commands. HPSPICE Elements and Device Models Manual Describes standard models you can use when simulating your circuit designs in HSPICE, including passive devices, diodes, JFET and MESFET devices, and BJT devices. HPSPICE MOSFET Models Manual Describes standard MOSFET models you can use when simulating your circuit designs in HSPICE. HSPICE RF Manual Describes a special set of analysis and design capabilities added to HSPICE to support RF and high-speed circuit design. AvanWaves User Guide Describes the AvanWaves tool, which you can use to display waveforms generated during HSPICE circuit design simulation. HSPICE® Simulation and Analysis User Guide X-2005.06 xxv About This Manual Searching Across the HSPICE Documentation Set Manual Description HSPICE Quick Reference Guide Provides key reference information for using HSPICE, including syntax and descriptions for commands, options, parameters, elements, and more. HSPICE Device Models Quick Reference Guide Provides key reference information for using HSPICE device models, including passive devices, diodes, JFET and MESFET devices, and BJT devices. Searching Across the HSPICE Documentation Set Synopsys includes an index with your HSPICE documentation that lets you search the entire HSPICE documentation set for a particular topic or keyword. In a single operation, you can instantly generate a list of hits that are hyperlinked to the occurrences of your search term. For information on how to perform searches across multiple PDF documents, see the HSPICE release notes (available on SolvNet at http://solvnet.synopsys.com) or the Adobe Reader online help. Note: To use this feature, the HSPICE documentation files, the Index directory, and the index.pdx file must reside in the same directory. (This is the default installation for Synopsys documentation.) Also, Adobe Acrobat must be invoked as a standalone application rather than as a plug-in to your web browser. Other Related Publications For additional information about HSPICE, see: xxvi ■ The HSPICE release notes, available on SolvNet (see Accessing SolvNet on page xxviii) ■ Documentation on the Web, which provides HTML and PDF documents and is available through SolvNet at http://solvnet.synopsys.com ■ The Synopsys MediaDocs Shop, from which you can order printed copies of Synopsys documents, at http://mediadocs.synopsys.com HSPICE® Simulation and Analysis User Guide X-2005.06 About This Manual Conventions You might also want to refer to the documentation for the following related Synopsys products: ■ CosmosScope ■ Aurora ■ Raphael ■ VCS Conventions The following conventions are used in Synopsys documentation: Convention Description Courier Indicates command syntax. Italic Indicates a user-defined value, such as object_name. Bold Indicates user input—text you type verbatim—in syntax and examples. [] Denotes optional parameters, such as write_file [-f filename] ... Indicates that a parameter can be repeated as many times as necessary: pin1 [pin2 ... pinN] | Indicates a choice among alternatives, such as low | medium | high \ Indicates a continuation of a command line. / Indicates levels of directory structure. Edit > Copy Indicates a path to a menu command, such as opening the Edit menu and choosing Copy. Control-c Indicates a keyboard combination, such as holding down the Control key and pressing c. HSPICE® Simulation and Analysis User Guide X-2005.06 xxvii About This Manual Customer Support Customer Support Customer support is available through SolvNet online customer support and through contacting the Synopsys Technical Support Center. Accessing SolvNet SolvNet includes an electronic knowledge base of technical articles and answers to frequently asked questions about Synopsys tools. SolvNet also gives you access to a wide range of Synopsys online services, which include downloading software, viewing Documentation on the Web, and entering a call to the Support Center. To access SolvNet: 1. Go to the SolvNet Web page at http://solvnet.synopsys.com. 2. If prompted, enter your user name and password. (If you do not have a Synopsys user name and password, follow the instructions to register with SolvNet.) If you need help using SolvNet, click SolvNet Help in the Support Resources section. Contacting the Synopsys Technical Support Center If you have problems, questions, or suggestions, you can contact the Synopsys Technical Support Center in the following ways: xxviii ■ Open a call to your local support center from the Web by going to http://solvnet.synopsys.com (Synopsys user name and password required), then clicking “Enter a Call to the Support Center.” ■ Send an e-mail message to your local support center. • E-mail [email protected] from within North America. • Find other local support center e-mail addresses at http://www.synopsys.com/support/support_ctr. HSPICE® Simulation and Analysis User Guide X-2005.06 About This Manual Customer Support ■ 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 X-2005.06 xxix About This Manual Customer Support xxx HSPICE® Simulation and Analysis User Guide X-2005.06 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). HSPICE® Simulation and Analysis User Guide X-2005.09 1 1: Overview HSPICE Varieties Figure 1 Synopsys HSPICE or HSPICE RF Design Features Transmission Line Signal Integrity Monte Carlo Worst-Case Analysis HSPICE or HSPICE RF Photocurrent/ Radiation Effects Incremental Optimization Circuit Cell Optimization Cell Characterization 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. 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 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 2 HSPICE® Simulation and Analysis User Guide X-2005.09 1: Overview Features 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 also supports some (but not all) of these features. For descriptions of features that HSPICE RF supports, but HSPICE does not, see the HSPICE RF User Guide. The HSPICE RF User Guide also indicates which features of HSPICE are supported in HSPICE RF. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 3 1: Overview Features 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). Figure 2 Synopsys HSPICE or HSPICE RF Circuit Analysis Types Parametric Operating Point Pole-Zero Monte Carlo Optimization HSPICE or HSPICE RF Monte Carlo Data Driven Frequency Transient S-parameter Monte Carlo analysis supported in Synopsys HSPICE only 4 Optimization Monte Carlo Data Driven Monte Carlo Optimization Mixed AC/Transient Data Driven HSPICE® Simulation and Analysis User Guide X-2005.09 1: Overview Features Figure 3 Synopsys HSPICE Modeling Technologies SPICE 40+ Industrial and Academic Models Magnetics MOS BJT IBIS Lossy Transmission Lines Mixed Signal Device Models Diode SOI Common Model Interface JFET/ GaAsFET Tunnel Diode 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 statement. ■ Statistical analysis – SWEEP MONTE analysis statement (HSPICE only). HSPICE® Simulation and Analysis User Guide X-2005.09 5 1: Overview Simulation Structure ■ 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. Figure 4 Simulation Program Structure Simulation Experiment Single point Analysis Initial Conditions Optimization Circuit Transient Sweep Results Analysis DC Timing Violations Statistical Worst Case 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: 6 ■ process ■ voltage HSPICE® Simulation and Analysis User Guide X-2005.09 1: Overview Simulation Structure ■ 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: ■ Process variation – Monte Carlo or worst-case model parameter variation (HSPICE only). ■ Element variation – Monte Carlo (HSPICE only) or element parameter sweeps. ■ 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 X-2005.09 7 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 X-2005.09 1: Overview Simulation Structure 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 DOS command line, 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 for HSPICE is AvanWaves. AvanWaves output display and analysis includes a graphical user interface. Use the mouse to select options, and to execute commands, in the AvanWaves windows. Refer to the AvanWaves User Guide for instructions about how to use AvanWaves. The default waveform display tool for HSPICE RF is 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 X-2005.09 9 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 X-2005.09 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 manual. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 11 2: Setup and Simulation Setting Environment Variables 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 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 12 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Standard Input Files 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 13 2: Setup and Simulation Standard Input Files 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# 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. 14 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Standard Input Files 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 15 2: Setup and Simulation Standard Output Files Standard Output Files This section describes the standard output files from HSPICE or HSPICE RF. The various types of output files produced are listed in Table 2. Table 2 HSPICE Output Files and Suffixes 16 Output File Type Extension AC analysis measurement results .ma# 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# Hardcopy graph data (from meta.cfg PRTDEFAULT) .gr# † HBLSP analysis extraction results .p2d# HBLSP large-signal analysis results (from .PROBE statement) .ls#. HBLSP small-signal analysis results (from .PROBE statement) .ss# HBLSP large-signal analysis results (from .PRINT statement) .printls# HBLSP small-signal analysis results (from .PRINT statement) .printss# Operating point information (from .OPTION OPFILE statement) .dp# Operating point node voltages (initial conditions) .ic# HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Standard Output Files Table 2 HSPICE Output Files and Suffixes (Continued) Output File Type Extension 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# # Either a sweep number, or a hardcopy file number. For .ac#, .dp#, .dm#, .ic#, .st#, .sw#, and .tr# files, # is from 0 through 9999. † 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. In HSPICE RF, you cannot replicate output commands within subcircuit (subckt) definitions. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 17 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. HBLSP Analysis Extraction Results File HSPICE RF writes HBSLP analysis extraction results to file <output_file>.p2d#, where # is 0-9999, according to your specifications following the .HBLSP statement. These results list the extracted large- and small-signal S parameters and noise parameters. 18 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Standard Output Files HBLSP Analysis Results File HSPICE RF writes HBSLP large-signal analysis results to file <output_file>.ls#, and small-signal analysis results to file <output_file>.ss#, where # is 0-9999, according to your specifications following the .PROBE statement. These results are viewable in CosmosScope. HBLSP Analysis Print Information File HSPICE RF writes HBSLP large-signal analysis results to file <output_file>.printls#, and small-signal analysis results to file <output_file>.printss#, where # is 0-9999, according to your specifications following the .PRINT statement. Operating Point Information File HSPICE writes operating point information to file <design>.dp# when the input file includes an .OPTION OPFILE=1 statement. Operating Point Node Voltages File HSPICE writes operating point node voltages to file <output_file>.ic#, where # is 0-9999, when the input file includes a .SAVE statement. These node voltages are the DC operating point initial conditions. Output Listing File The output listing is a text file. It can be named <output_file> (no file extension), <output_file>.lis, or with a file extension that you specify, depending on which format you use to start the simulation. For HSPICE RF, the output is a table of simulation results. If the output is text (the default), the output is HTML, which you can view in a web browser. If you set the -a command-line argument, this table displays ASCII text output to stdout, which you can redirect to an output file. HSPICE® Simulation and Analysis User Guide X-2005.09 19 2: Setup and Simulation Standard Output Files The output file includes the following information: ■ Name of the simulator used. ■ Version of the HSPICE simulator used (HSPICE RF does not produce backward-compatible .lis files). ■ Synopsys message block. ■ Input filename. ■ User name. ■ License details. ■ Copy of the input netlist file. ■ Node count. ■ Operating point parameters. ■ Details of the volt drop, current, and power for each source and subcircuit. ■ Low-resolution plots, originating from a .PLOT statement. ■ Results of a .PRINT statement. ■ Results of the .OPTION statements. The Synopsys interactive waveform display tool, CosmosScope, can display both the text simulation results, and binary output, in the X-window environment. 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. 20 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Standard Output Files 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 command-line argument. This file lists the numerical results of transient analysis. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 21 2: Setup and Simulation Starting HSPICE Starting HSPICE Use the following syntax to start HSPICE: hspice <-i <path/input_file>> <-o <path/output_file>> <-n number> <-html <path/html_file>> <-b> <-d> <-mt number> <-I> HSPICE accepts these command-line arguments: Arguments Description -i Specifies the input netlist filename for which an extension <.ext> is path/input_f optional. If you do not specify an input filename extension in the ile command, HSPICE searches for a <input_file>.sp file. HSPICE uses the input filename as the root for the output files. HSPICE also checks for an initial conditions file (.ic) that has the input file root name. The following is an example of an input filename: /usr/sim/work/rb_design.sp In this filename: • /usr/sim/work/ is the directory path to the design. • rb_design is the design root name. • .sp is the filename suffix. -o path/output_file Name of the output file. If you do not specify an extension, HSPICE assigns .lis. Everything up to the final period is the root filename, and everything after the last period is the filename extension. • If you either do not use this option or you use it without specifying a filename, HSPICE uses the output root filename specified in the -html option. • If you do not specify an output filename in either this or the -html option, HSPICE uses the input root filename as the output file root filename. • If you include the .lis extension in the filename that you enter using this option, then HSPICE does not append another .lis extension to the root filename of the output file. • If you do not specify an output filename, HSPICE directs output to stdout. -n number 22 Specifies the starting number for numbering output data file revisions (output_file.tr#, output_file.ac#, output_file.sw#, where # is between 0 and 9999.). HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Starting HSPICE Arguments Description -html path/html_file Specifies an HTML output file. • If you do not specify a path, HSPICE saves the HTML output file in the same directory that you specified in the -o option. • If you do not specify an -o option, HSPICE saves the HTML output in the working directory. • If you do not specify an output filename in either the -o or -html option, then HSPICE uses the input root filename as the output file root filename. -b (PC) Batch processing switch for Windows platforms only. -d (UNIX) Displays the content of .st0 files on screen while running HSPICE. For example, to show the status during simulation. At he prompt, you could also enter: tail -f *.st0. -mt number Number of processors for multi-threaded simulation. • If you omit the number, an error message results. You must include this parameter. • If you specify a number that is larger than the number of available CPUs, then HSPICE sets the number of threads equal to the number of available CPUs. -I Interactive mode. Redirecting Output Use the following syntax to redirect the output to a file instead of to stdout: hspice input_file <-n number> > output_file For example: hspice demo.sp -n 7 > demo.out Where: demo.sp is the input netlist file. The .sp extension is optional. -n 7 starts the output data file revision numbers at 7; for example: demo.tr7, demo.ac7, demo.sw7, and so forth. > redirects the program output listing to file demo.out. HSPICE® Simulation and Analysis User Guide X-2005.09 23 2: Setup and Simulation Running an HSPICE Simulation Running an HSPICE Simulation Perform these steps to run a HSPICE simulation. 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. 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. 24 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Running an HSPICE Simulation (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 You can find the complete netlist for this example in the following directory: $installdir/demo/hspice/apps/inv_ex1.sp 6. Library input. HSPICE reads any files that you specified in .INCLUDE and .LIB statements. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 25 2: Setup and Simulation Interactive Simulation 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. Interactive Simulation To invoke HSPICE in interactive mode, enter: hspice -I You can then use other HSPICE commands to help you simulate circuits interactively. You can also use the help command for detailed information about a command. HSPICE 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> To run the command you have saved in a command file, enter the following line: hspice -I -L command.cmd Examples of Starting HSPICE The following are some additional examples of commands to start running HSPICE. ■ hspice -i demo.sp demo is the root filename. Without the -o option and without redirection, HSPICE does not generate an output listing file. ■ hspice -i demo.sp -o demo demo is the output file root name (designated with the -o option). Output files are named demo.lis, demo.tr0, demo.st0, and demo.ic0. 26 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Examples of Starting HSPICE ■ hspice -i rbdir/demo.sp demo is the root name. HSPICE writes the demo.lis, demo.tr0, and demo.st0 output files into the directory where you executed the HSPICE command. It also writes the demo.ic0 output file into the same directory as the input source—that is, rbdir. ■ hspice -i a.b.sp a.b is the root name. The output files are ./a.b.lis, ./a.b.tr0, ./a.b.st0, and ./a.b.ic0. ■ hspice -i a.b -o d.e a.b is the root name for the input file. d.e is the root for output file names, except for the .ic file, to which HSPICE assigns the a.b input file root name. The output files are d.e.lis, d.e.tr0, d.e.st0, and a.b.ic0. ■ hspice -i a.b.sp -o outdir/d.e a.b is the root for the .ic0 file. HSPICE writes the .ic0 file into a file named a.b.ic0. d.e is the root for other output files. Output files are outdir/d.e.lis, outdir/d.e.tr0, and outdir/d.e.st0. ■ hspice -i indir/a.b.sp -o outdir/d.e.lis a.b is the root for the .ic file. HSPICE writes the .ic0 file into a file named indir/a.b.ic0. d.e is the root for the output files. ■ hspice test.sp -o test.lis -html test.html This command creates output file in both .lis and .html format, after simulating the test.sp input netlist. ■ hspice test.sp -html test.html This command creates only a .html output file, after simulating the test.sp input netlist. ■ hspice test.sp -o test.lis This command creates only a .lis output file, after simulating the test.sp input netlist. HSPICE® Simulation and Analysis User Guide X-2005.09 27 2: Setup and Simulation Starting HSPICE RF ■ hspice -i test.sp -o -html outdir/a.html This command creates output files in both .lis and .html format. Both files are in the outdir directory, and their root filename is a. ■ hspice -i test.sp -o out1/a.lis -html out2/b.html This command creates output files in both .lis and .html format. The .lis file is in the out1 directory, and its root filename is a. The .html file is in the out2 directory, and its root filename is b. Starting HSPICE RF Use the following syntax to start HSPICE RF: hspicerf [-a] inputfile [outputfile] [-h] [-v] HSPICE RF accepts these command-line arguments: Argument Description -a Generates output to sdout in ASCII format. For example, % hspicerf -a ckt.in You can redirect the ASCII output to another file. For example: % hspicerf -a ckt.in > xt Output from a .PRINT command goes to an ASCII file with a .print# or .printac# file extension. inputfile The name of the input netlist. outputfile The name of the output listing file. • If specified, the simulation output is written to this file and given a .lis file extension. For example, % hspicerf ckt.in xt automatically sets -a and generates output to xt.lis. • If not specified (the default), an html directory is created and the simulation output is written to an hspicerf.html file in that directory. For example, % hspicerf ckt.in generates output to html/hspicerf.html. Use your web browser to view this file. 28 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Improving Simulation Performance with Multithreading Argument Description -h Returns a help message. -v Returns version information. Improving Simulation Performance with Multithreading 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. Running HSPICE-MT On UNIX platforms, use this syntax to run HSPICE-MT: hspice -mt number -i input_file -o output_file On Windows platforms, use this syntax to run HSPICE-MT: hspice_mt.exe -mt number -i input_file -o output_file For a description of the options shown in the syntax lines above, see section Starting HSPICE on page 22. 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 HSPUI (HSPICE User Interface): 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. HSPICE® Simulation and Analysis User Guide X-2005.09 29 2: Setup and Simulation Simulating in Client/Server Mode 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 machine. Ideally, assuming Toverhead = 0, you can achieve a speedup of: T1cpu/(0.2T1cpu + 0.8T1cpu/2cpus) = 1.67 The typical Tparallel value is 0.6 to 0.7 for moderate to large circuits. Simulating 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. 1. Enter Client/Server mode: hspice -C This step creates an HSPICE server, and checks out an HSPICE license. 2. Simulate your netlist hspice -C input_file This step runs simulation without checking out an HSPICE license. 30 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Simulating in Client/Server Mode Note: This mode also supports other HSPICE command line options. For a description of these options shown, see section Starting HSPICE on page 22. 3. Exit Client/Server mode hspice -C -K This step releases the HSPICE license and exits HSPICE. 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. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 31 2: Setup and Simulation Simulating in Client/Server Mode 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. 32 HSPICE® Simulation and Analysis User Guide X-2005.09 2: Setup and Simulation Simulating with Stand-alone .MEASURE Calculations Simulating with Stand-alone .MEASURE Calculations When you want to calculate new measurements from previous simulation results produced by HSPICE, you can use the following mode to rerun HSPICE: hspice -meas measurefile -i wavefile <-o <outputfile>> Argument Description -meas measurefile This fomat is similar to the HSPICE netlist format. The first line is a comment line, and the last line is an .END statement. Seven commands are supported: • .MEASURE • .PARAM • .TEMP • .OPTION • .DATA • .ENDDATA • .END Note: The .DATA statement in the measure file must be consistent with the .DATA statement in the wavefile. The .OPTION statement support four types: • MEASFAIL • NUMDGT • INGOLD • MEASDGT Warnings are issued if other options or statements are used. Wave files formatted as PSF and CSDF are not supported. -i wavefile This argument specifies the *.tr#, *.ac#, and *.sw# files produced by HSPICE. Wave files formatted as PSF are not supported. -o outputfile Specifies the same output files as HSPICE. Some case results are different from the measure result HSPICE produces due to an accuracy problem. HSPICE® Simulation and Analysis User Guide X-2005.09 33 2: Setup and Simulation Simulating with Stand-alone .MEASURE Calculations 34 HSPICE® Simulation and Analysis User Guide X-2005.09 3 Input Netlist and Data Entry 3 Describes the input netlist file and methods of entering data. For descriptions of individual HSPICE commands referenced in this chapter, see 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. HSPICE® Simulation and Analysis User Guide X-2005.09 35 3: Input Netlist and Data Entry Input Netlist File Guidelines 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. 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 38. ■ 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 example, 2**5 represents two to the fifth power (25) ■ To continue all HSPICE or HSPICE RF statements, including quoted strings (such as paths and algebraics), use a backslash (\) or a double backslash (\\) at the end of the line that you want to continue. • 36 A single backslash preserves white space. HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Guidelines ■ Names must begin with an alphabetic character, but thereafter can contain numbers and the following characters: ! # $ % * + / < > [ ] _ { } : ; ? | . , • When you use an asterisk (*) or a question mark (?) with a .PRINT, .PROBE, .PLOT (HSPICE), .GRAPH, .LPRINT (HSPICE RF), or .CHECK (HSPICE RF) statement, HSPICE or HSPICE RF uses the character as a wildcard. For additional information, see Using Wildcards on Node Names on page 51. • When you use curly brackets ( { } ), HSPICE converts them to square brackets ( [ ] ) automatically. • 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. HSPICE® Simulation and Analysis User Guide X-2005.09 37 3: Input Netlist and Data Entry Input Netlist File Guidelines First Character The first character in every line specifies how HSPICE and HSPICE RF interprets the remaining line. Table 3 lists 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 Delimiters 38 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Guidelines 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 50. ■ 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 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 HSPICE® Simulation and Analysis User Guide X-2005.09 39 3: Input Netlist and Data Entry Input Netlist File Guidelines Table 4 Element Identifiers (Continued) Letter (First Char) Element Example Line 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 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 40 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Guidelines 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 Note: 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. real. Table 5 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 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 HSPICE® Simulation and Analysis User Guide X-2005.09 41 3: Input Netlist and Data Entry Input Netlist File Guidelines 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 (20-18mps), 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. 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: ! # $ % [ ] _ 42 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Guidelines ■ 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, 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. Schematic Netlists HSPICE or HSPICE RF typically use netlisters to generate circuits from schematics, and accept either hierarchical or flat netlists. The normal SPICE netlisters flatten all subcircuits, and rename all nodes to numbers. Avoid flat netlisters if possible. The process of creating a schematic involves: ■ Symbol creation with a symbol editor. ■ Circuit encapsulation. ■ Property creation. ■ Symbol placement. HSPICE® Simulation and Analysis User Guide X-2005.09 43 3: Input Netlist and Data Entry Input Netlist File Guidelines ■ 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. Output .PRINT, .PLOT, .GRAPH, .PROBE .MEASURE Statements to output variables. .INCLUDE General include files. .MALIAS Assigns an alias to a diode, BJT, JFET, or MOSFET. .MODEL Element model descriptions. .LIB Library. Library, Model and File Inclusion 44 Statement to evaluate and report userdefined functions of a circuit. HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition Table 6 Input Netlist File Sections (Continued) Sections Examples Definition .OPTION SEARCH Search path for libraries and included files. .PROTECT and .UNPROTECT Control printback to output listing. Alter blocks .ALIAS .ALTER .DELETE LIB Renames a previous model. Sequence for in-line case analysis. Removes previous library selection. End of netlist .END Required statement; end of netlist. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 Element and input control statements Analysis/output control statements 45 3: Input Netlist and Data Entry Input Netlist File Composition 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. 3. 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 ***** .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 HSPICE Command Reference manual. 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. 46 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition 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 (#) 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. 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 a space or comma, unless that character is a units comment (scale factor) to a number. You can 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 .MODEL n1 * This is + LEVEL = a comment line NMOS $ this is an example of an inline comment a comment line and the following line is a continuation 3 HSPICE® Simulation and Analysis User Guide X-2005.09 47 3: Input Netlist and Data Entry Input Netlist File Composition 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. 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 ... 48 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> HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition Table 7 Element Parameters (Continued) Parameter Description 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 49 3: Input Netlist and Data Entry Input Netlist File Composition 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). 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 file. 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. 50 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition In addition to letters and digits, node names can include the following characters: +, -, *, /, $, #, [], !, <>, _, % 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> 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 X-2005.09 51 3: Input Netlist and Data Entry Input Netlist File Composition Wildcards must begin with a letter or a number. For example: .PROBE v(*) correct format .PROBE * incorrect format .PROBE x* 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. You must create an .admrc file to use these wildcards. ■ Probe all top-level in a design hierarchy. .PROBE v(*) ■ Probe all first-level nodes, where zero-level are top-level nodes whose names start with a, and all nodes at all levels below it. For example: a1, a2, a3, a00, ayz. .PROBE v(a*) ■ Print all first-level nodes, where zero-level are top-level nodes, and all nodes at all levels below it. For example: X1.A, X4.554, Xab.abc123. .PRINT v(*.*) ■ Probe all first-level nodes that start with x, where zero-level are top-level nodes, and all nodes at all levels below it. For example: x1.A, x4.554, xab.abc123. This example creates only waveform data, without an ASCII table of results. .PROBE v(x*.*) 52 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition ■ Print all second-level nodes. For example: x1.x2.a, xab.xdff.in. .PRINT v(x*.*.*) ■ 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 48). 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. HSPICE® Simulation and Analysis User Guide X-2005.09 53 3: Input Netlist and Data Entry Input Netlist File Composition 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 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 54. 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) 54 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 55 3: Input Netlist and Data Entry Input Netlist File Composition 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. 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: 56 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition ■ 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.”. 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 1. 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. 2. A library cannot contain a call to a library of its own entry name, within the same library file. 3. A HSPICE or HSPICE RF library cannot contain the .END statement. 4. .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. HSPICE® Simulation and Analysis User Guide X-2005.09 57 3: Input Netlist and Data Entry Input Netlist File Composition 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. 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 HSPICE Command Reference manual. HSPICE or HSPICE RF supports the following predefined analysis parameters: 58 ■ Temperature functions (fn) ■ Optimization guess/range HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Input Netlist File Composition HSPICE also supports the following predefined parameter types, that HSPICE RF does not support: ■ frequency ■ time ■ Monte Carlo functions 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. 1. 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. 2. 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. 3. 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. 4. 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. 5. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 59 3: Input Netlist and Data Entry Input Netlist File Composition 6. Each .ALTER simulation run prints only the actual altered input. A special .ALTER title identifies the run. 7. .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. Using Multiple .ALTER Blocks This section does not apply to HSPICE RF. 1. 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. 2. 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. 3. HSPICE then uses these statements to modify the input netlist file. 4. HSPICE then resimulates the circuit. 5. For each additional .ALTER statement, HSPICE performs the simulation that precedes the first .ALTER statement. 6. 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. 60 HSPICE® Simulation and Analysis User Guide X-2005.09 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, or select different model cards 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 ■ 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) ). HSPICE® Simulation and Analysis User Guide X-2005.09 61 3: Input Netlist and Data Entry Input Netlist File Composition ■ 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, .SUBCKT, .ENDS, .MACRO, .EOM, .GLOB AL, .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, but you cannot include subcircuits in IF-ELSEIF-ELSE statements. ■ However, 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 an unlimited number of ELSEIF statements within an IFELSE block. ■ You cannot include sweep parameters or simulation results within an IFELSE 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 62 HSPICE® Simulation and Analysis User Guide X-2005.09 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 X-2005.09 63 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 64 EXPANDED HSPICE® Simulation and Analysis User Guide X-2005.09 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. 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 X-2005.09 65 3: Input Netlist and Data Entry Using Subcircuits 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 This section does not apply to HSPICE RF. If a subcircuit call is in a data file that does not describe the subcircuit, HSPICE automatically searches the: 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. 66 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Subcircuit Call Statement Discrete Device Libraries 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 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 48 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. HSPICE® Simulation and Analysis User Guide X-2005.09 67 3: Input Netlist and Data Entry Subcircuit Call Statement Discrete Device Libraries 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. ■ 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. 68 HSPICE® Simulation and Analysis User Guide X-2005.09 3: Input Netlist and Data Entry Subcircuit Call Statement Discrete Device Libraries Figure 12 Vendor Library Usage x1 in out vdd vss buffer_f .OPTION search = ‘/usr/lib/vendor’ /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 /usr/lib/vendor/buffer.inc /usr/lib/vendor/model.dat .model nch nmos level = 28 + xl = vendor_xl ... .macro buffer in out vdd vss m1 out in vdd vdd nch w = 10 l = 1 ... 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 X-2005.09 69 3: Input Netlist and Data Entry Subcircuit Call Statement Discrete Device Libraries 70 HSPICE® Simulation and Analysis User Guide X-2005.09 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 the HSPICE 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 X-2005.09 71 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’ ... 72 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. Refer to the “Using 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: • • • • • 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 X-2005.09 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 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 HSPICE® Simulation and Analysis User Guide X-2005.09 73 4: Elements Passive Elements 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). 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 > 74 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Passive Elements Parameter Description TC1, TC2 Temperature coefficient. W Resistor width. 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 X-2005.09 75 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. • 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. FBASE 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 76 HSPICE® Simulation and Analysis User Guide X-2005.09 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. HSPICE® Simulation and Analysis User Guide X-2005.09 77 4: Elements Passive Elements Parameter Description TC1 First-order temperature coefficient for the capacitor. Refer to Chapter 2, “Using Passive Device Models”, in the HSPICE Elements and Device Models Manual for temperature-dependant relations. TC2 Second-order temperature coefficient for the capacitor. 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 78 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Passive Elements Parameter Description 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. ■ 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 79 4: Elements Passive Elements 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 Linear Capacitors Cxxx node1 node2 < modelname > < C = > value < TC1 = val > + < TC2 = val > <W = val > < L = val > < DTEMP = val > + < M = val > < SCALE = val > < IC = val > 80 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Passive Elements Parameter Description 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: ■ Cbypass is a straightforward, 10-picofarad (PF) capacitor. ■ C1, which calls the CBX model, does not have a constant capacitance. ■ 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>> HSPICE® Simulation and Analysis User Guide X-2005.09 81 4: Elements Passive Elements 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. Example C1 1 2 C='1e-6 - HERTZ/1e16' CONVOLUTION=1 fbase=10 + fmax=30meg 82 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Passive Elements 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. HSPICE® Simulation and Analysis User Guide X-2005.09 83 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)) 84 HSPICE® Simulation and Analysis User Guide X-2005.09 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...> HSPICE® Simulation and Analysis User Guide X-2005.09 85 4: Elements Passive Elements 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. TC1 First-order temperature coefficient for the inductor. Refer to Chapter 2, “Using Passive Device Models”, 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: • • • • • 86 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Passive Elements Parameter Description L = ‘equation’ Inductance at room temperature, specified as: • a function of any node voltages • a function of branch currents • any independent variables such as time, hertz, and temper LTYPE 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. 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 Chapter 2, “Using Passive Device Models”, 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 Chapter 2 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 HSPICE® Simulation and Analysis User Guide X-2005.09 87 4: Elements Passive Elements 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 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 Mutual core form: Kaaa Lbbb <Lccc ... <Lddd>> mname <MAG = magnetization> 88 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Passive Elements Parameter Description 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. Kaaa Saturable core element name. Must begin with K, followed by up to 1023 alphanumeric characters. 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. mname Saturable core model name. See Chapter 2, “Using Passive Device Models”, in the HSPICE Elements and Device Models Manual for model information. MAG = magnetization 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 Chapter 2, “Using Passive Device Models”, in the HSPICE Elements and Device Models Manual). 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 89 4: Elements Passive Elements Example 1 The Lin and Lout inductors are coupled, with a coefficient of 0.9. K1 Lin Lout 0.9 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 Kxxxx Li Lj <k=> IDEAL Ideal transformers use 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 interms 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 90 HSPICE® Simulation and Analysis User Guide X-2005.09 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 HSPICE® Simulation and Analysis User Guide X-2005.09 91 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> 92 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 X-2005.09 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=valule> + <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. • 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 X-2005.09 93 4: Elements Passive Elements Parameter Description FBASE 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. • 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. Example L1 1 2 L='0.5n + 0.5n/(1 + HERTZ/1e8)' CONVOLUTION=1 fbase=10 + fmax=30meg AC Choke Inductors 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 HSPICE 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 using HSPICE RF, either set them to ANALOG mode, or invoke the SIM_RAIL option: .OPTION SIM_ANALOG = “L1” or .OPTION SIM_RAIL = ON 94 HSPICE® Simulation and Analysis User Guide X-2005.09 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 X-2005.09 95 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. 96 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Active Elements Example 1 The D1 diode, with anode and cathode, connects to nodes 1 and 2. Diode1 specifies the diode model. D1 1 2 diode1 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. HSPICE® Simulation and Analysis User Guide X-2005.09 97 4: Elements Active Elements Parameter Description area, Emitter area multiplying factor, which affects currents, resistances, and AREA = area capacitances. Default = 1.0. OFF Sets initial condition for this element to OFF, in DC analysis. Default=ON. 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 98 ■ The collector connects to node 1. ■ The base connects to node 2. ■ The emitter connects to node 3. ■ model_1 references the BJT model. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Active Elements Example 2 In the following Qopamp1 BJT element: Qopamp1 c1 b3 e2 s 1stagepnp AREA = 1.5 AREAB = 2.5 AREAC = 3.0 ■ 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. ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 99 4: Elements Active Elements 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> 100 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Active Elements Parameter Description 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 ■ The drain connects to the d1 node. ■ The source connects to the g3 node. ■ The gate connects to the s2 node. ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 101 4: Elements Active Elements ■ 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...> 102 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 L MOSFET channel length, in meters. This parameter overrides .OPTION DEFL. Default = DEFL, with a maximum value of 0.1m. W MOSFET channel width, in meters. This parameter overrides DEFW in an .OPTION statement. Default = DEFW. AD Drain diffusion area. Overrides DEFAD in the .OPTION statement. Default = DEFAD, if you set the ACM = 0 model parameter. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Active Elements Parameter Description AS Source diffusion area. Overrides DEFAS in the .OPTION statement. 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 DEFNRS in the .OPTION statement. 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, Initial voltage across external drain and source (vds), gate and source vbs (vgs), and bulk and source terminals (vbs). Use these arguments with .TRAN UIC. .IC statements override these values. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 103 4: Elements Active Elements Parameter Description 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 = 4.0 104 ■ The drain connects to the driver node. ■ The gate connects to the in node. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines ■ 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 Wxxx i1 i2 ... iN iR o1 o2 ... oN oR N=val L=val + TABLEMODEL=name Parameter Description N Number of signal conductors (excluding the reference conductor). i1...iN Node names for the near-end signal-conductor terminal. iR Node name for the near-end reference-conductor terminal. HSPICE® Simulation and Analysis User Guide X-2005.09 105 4: Elements Transmission Lines Parameter Description o1...oN Node names for the far-end signal-conductor terminal. oR Node name for the far-end reference-conductor terminal. L Length of the transmission line. TABLEMODEL Name of the frequency-dependent tabular model. The W element supports five different formats to specify the transmission line properties: ■ ■ Model 1: RLGC-Model specification. • Internally specified in a .model statement. • Externally specified in a different file. 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 = fname> <COORD=0|DESCART|1|POLAR> + N = val L = val U Model form: Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <Umodel = mname> N = val L = val 106 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines Field solver form: Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <FSmodel = mname> 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 = mname> <NODEMAP=XiYj...> N = val L = val 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 = fname File name reference for the file containing the RLGC information for the transmission lines (for syntax, see Chapter 3, “Using Transmission Lines,” in the HSPICE Signal Integrity Guide). COORD Invokes the polar field solver only if COORD=1 or COORD=POLAR. ORIGIN Should be (radius, degree) for the polar field solver. HSPICE® Simulation and Analysis User Guide X-2005.09 107 4: Elements Transmission Lines Parameter Description Umodel = mname 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 = mname Internal field solver model name. References the PETL internal field solver, as the source of the transmission-line characteristics (for syntax, see the HSPICE Signal Integrity Guide). 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, the HSPICE Signal Integrity Guide). 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 = 10 108 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 109 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 + _ [i2]1 [i2]2 . . . Reference conductor 2.1 2.2 [i2]N 2.N [v2]N + _ 2’ x 0 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 110 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. refout Ground reference for the output signal. Z0 Characteristic impedance of the transmission line. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines 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 ■ 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 X-2005.09 111 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 ) ] A j ( ωt – βx ) B 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 β l becomes the following equation: l β l = ω LC ⋅ l = ω ----vp 112 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines This is equivalent to an ideal delay with the following value: τ= l = LC ⋅ l vp τ : absolute time delay (sec) l : physical length (L ) (meters ) v p : phase velocity (meters / sec) Using standard distance=velocity*time relationships, the HSPICE T element parameter values are related to these terms according to: vp = f ⋅ λ = 1 td f : frequency λ : wavelength t d : relative time delay (TD) (sec/ meter ) τ= l l lλ = td ⋅ l = = = LC ⋅ l vp f ⋅λ f l : physical length (L ) (meters ) l λ : normalized length (NL ) f : frequency at NL (F) (Hz) τ = TD ⋅ L = NL = LC ⋅ L F HSPICE therefore allows you to specify a transmission line in three different ways: ■ Z0, TD, L ■ Z0, NL, F ■ L, with L and C LC values taken from a U model. HSPICE® Simulation and Analysis User Guide X-2005.09 113 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 = 5 114 ■ Both signal references are grounded. ■ umodel_RG58 references the U-model. ■ The transmission line is 5 meters long. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines 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 ■ 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 Chapter 2 of the HSPICE Signal Integrity Guide. HSPICE® Simulation and Analysis User Guide X-2005.09 115 4: Elements Transmission Lines 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]> + <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> 116 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines Parameter Description nd1 nd2 ... ndN Nodes of an S element (see Figure 14). 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. 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 frequency-dependent 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: • S (scattering), the default • Y (admittance) • Z (impedance) HSPICE® Simulation and Analysis User Guide X-2005.09 117 4: Elements Transmission Lines Parameter Description Zo 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. 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 Pre-Conditioning S Parameters on page 122. 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 121 • 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 118 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. HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines Parameter Description INTERPOLATION The interpolation method: • STEP: piecewise step • SPLINE: b-spline curve fit • LINEAR: piecewise linear (default) INTDATTYP Data type for the linear interpolation of the complex data. • RI: real-imaginary based interpolation • DBA: dB-angle based interpolation • MA: magnitude-angle based interpolation (default) HIGHPASS 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 mixedsignal incident or reflected vector. The string must be an array of a letter and a number (Xn) where: • 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 X-2005.09 119 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 If 1, element generates thermal noise. If 0, element is considered noiseless. Default=0. 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. 120 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements Transmission Lines Figure 14 Terminal Node Notation . . . . . . . . . N+1 terminal system [vinc]1 [vinc]N [i]N [i]1 [vref]1 [vref]N ndN (+) [v]N nd1 (+) [v]1 (-) ndR (reference node) Frequency Table Model The Frequency Table Model is a generic model that you can use to describe frequency-varying behavior. Currently, the S element and .sp use this model. For a description of this model, see “Frequency Table Model” in Chapter 6, Linear N-Ports/Transmission Lines, in the HSPICE Elements and Device Models Manual. 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=0|1> keyword in the S model statement. HSPICE® Simulation and Analysis User Guide X-2005.09 121 4: Elements Transmission Lines 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: d θ Sij 1 d θ 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 j ωΤ 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 (1) Pre-Conditioning 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 adds kRref series resistance, to pre-condition S matrices: S ′ = [ kI + ( 2 – k ) S ] [ ( 2 + k ) I – kS ] ■ Rref is the reference impedance vector. ■ k is the pre-conditioning factor. –1 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 pre-conditioning factor, use the <PREFAC=val> keyword in the S model statement. The default pre-conditioning factor is 0.75. 122 HSPICE® Simulation and Analysis User Guide X-2005.09 4: Elements IBIS Buffers Figure 15 Pre-Conditioning S Parameters preconditioning S S kRref NMA stamp kRref Y’ Y’ Y 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. HSPICE® Simulation and Analysis User Guide X-2005.09 123 4: Elements IBIS Buffers Parameter Description 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 Command 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. 124 HSPICE® Simulation and Analysis User Guide X-2005.09 5 Sources and Stimuli 5 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. Some types of analysis use the associated analysis sources. For example, in a DC analysis, if you specify both DC and AC sources in one independent source element statement, HSPICE or HSPICE RF removes the AC source from the circuit for the DC analysis. If you specify an independent source for an AC, transient, and DC analysis, HSPICE or HSPICE RF removes transient sources, calculates the operating point, and removes DC sources for the AC analysis. Initial transient values always override the DC value. HSPICE® Simulation and Analysis User Guide X-2005.09 125 5: Sources and Stimuli Independent Source Elements 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. You can use parameters as values in independent sources. Do not use any of the reserved keywords to identify these parameters: AC PU ACI PULSE AM PWL DC R EXP RD PAT SFFM PE SIN PL Independent Source Element The general syntax for an independent source is: Vxxx n+ n- <<DC=> dcval> <tranfun> <AC=acmag> <acphase>> Ixxx n+ n- <<DC=> dcval> <tranfun> <AC=acmag> <acphase>> <M=val> 126 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. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Elements Parameter Description 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 127 5: Sources and Stimuli Independent Source Elements 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. 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, 128 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Elements Example 7 ISRC 23 21 AC 0.333 45.0 SFFM (0 1 10K 5 1K) Where, ■ 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 129 5: Sources and Stimuli Independent Source Elements 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. Transient Sources For transient analysis, you can specify the source as a function of time. The following functions are available: ■ pulse ■ exponential ■ damped sinusoidal ■ single-frequency FM ■ piecewise linear ■ pattern ■ PRBS (Pseudo Random-Bit Generator Source) 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. 130 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Elements 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. 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> HSPICE® Simulation and Analysis User Guide X-2005.09 131 5: Sources and Stimuli Independent Source Elements + $ **** 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. • 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_waveform> 132 (Transient analysis) Voltage or power source waveform. Any one of waveforms: AM, EXP, PULSE, PWL, SFFM, or SIN. Multiple transient descriptions are not allowed. HSPICE® Simulation and Analysis User Guide X-2005.09 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. • 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. <z0=val> (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 X-2005.09 133 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, .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. 134 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Independent Source Functions HSPICE or HSPICE RF uses the following types of independent source functions: ■ Pulse (PULSE function) ■ Sinusoidal (SIN function) ■ Exponential (EXP function) ■ Piecewise linear (PWL function) ■ Single-frequency FM (SFFM function) ■ Single-frequency AM (AM function) ■ Pattern (PATTERN 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. Pulse Source Function 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 X-2005.09 135 5: Sources and Stimuli Independent Source Functions The syntax for a pulse source, in an independent voltage or current source, is: 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 Time-Value Relationship for a PULSE Source 136 Time Value 0 v1 td v1 td + tr v2 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Table 8 Time-Value Relationship for a PULSE Source (Continued) Time Value td + tr + pw v2 td + tr + pw + tf v1 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. HSPICE® Simulation and Analysis User Guide X-2005.09 137 5: Sources and Stimuli Independent Source Functions ■ The pulse width is 20 nanoseconds. ■ The pulse period is 50 nanoseconds. You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/pulse.sp Figure 16 shows the result of simulating this netlist, in HSPICE or HSPICE RF. Figure 16 138 Pulse Source Function HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Sinusoidal Source Function HSPICE or HSPICE RF provides a damped sinusoidal source, 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 The syntax for a sinusoidal source in an independent voltage or current source is: 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 X-2005.09 139 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 2⋅Π⋅ϕ vo + va ⋅ SIN -------------------- 360 td to tstop vo + va ⋅ Exp [ – ( Time – td ) Þ 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 141 for a plot of the source output. 140 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Figure 17 Sinusoidal Source Function You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/sin.sp 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 HSPICE® Simulation and Analysis User Guide X-2005.09 141 5: Sources and Stimuli Independent Source Functions Exponential Source Function The general syntax for an exponential source, in an independent voltage or current source, is: Vxxx n+ n- EXP <(> v1 v2 <td1 <t1 <td2 <t2>>>> <)> Ixxx n+ n- EXP <(> v1 v2 <td1 <t1 <td2 <t2>>>> <)> 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. TSTEP is the printing increment, and TSTOP is the final time. 142 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions The following table of expressions defines the waveform shape: Table 11 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 X-2005.09 143 5: Sources and Stimuli Independent Source Functions Figure 18 Exponential Source Function You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/exp.sp This example shows an entire netlist, which contains an EXP voltage source. In this source: 144 ■ 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 80 ns, the waveform starts dropping to -4 V again, with a time constant of 40 ns. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Piecewise Linear (PWL) Source Function The general syntax for a piecewise linear source, in an independent voltage or current source, is: 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. TD=delay Time, in units of seconds, which specifies the length of time to delay (propagation delay) the piecewise linear function. HSPICE® Simulation and Analysis User Guide X-2005.09 145 5: Sources and Stimuli Independent Source Functions ■ 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. Example You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/pwl.sp 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. 146 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Figure 19 Results of Using the Repeat Function Data-Driven Piecewise Linear Source The general syntax for a data-driven piecewise linear source, in an independent voltage or current source, is: Vxxx n+ n- PWL (TIME, PV) Ixxx n+ n- PWL (TIME, PV) .DATA dataname TIME PV t1 v1 t2 v2 t3 v3 t4 v4 HSPICE® Simulation and Analysis User Guide X-2005.09 147 5: Sources and Stimuli Independent Source Functions .. .. .ENDDATA .TRAN DATA=datanam HSPICE RF does not support the data-driven PWL syntax. 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 You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/datadrive_pwl.sp 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. 148 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Single-Frequency FM Source Function The general syntax for including a single-frequency, frequency-modulated source in an independent voltage or current source is: 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 You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/sffm.sp This example shows an entire netlist, which contains a single-frequency, frequency-modulated voltage source. In this source. ■ The offset voltage is 0 volts. ■ The maximum voltage is 1 millivolt. HSPICE® Simulation and Analysis User Guide X-2005.09 149 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 20 150 Single Frequency FM Source HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Amplitude Modulation Source Function The general syntax for including a single-frequency, frequency-modulated source in an independent voltage or current source is: Vxxx n+ n- AM < (> sa oc fm fc <td> <)> 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 You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/amsrc.sp This example shows an entire netlist, which contains three amplitudemodulated voltage sources. HSPICE® Simulation and Analysis User Guide X-2005.09 151 5: Sources and Stimuli Independent Source Functions ■ ■ ■ 152 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 X-2005.09 5: Sources and Stimuli Independent Source Functions Figure 21 Amplitude Modulation Plot Pattern Source Function 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 “b-string.” HSPICE® Simulation and Analysis User Guide X-2005.09 153 5: Sources and Stimuli Independent Source Functions The following general syntax is for including a pattern source in an independent voltage or current source: Syntax Vxxx n+ n- PAT <(> vhi vlo td tr tf + <R=repeat> <)> Ixxx n+ n- PAT <(> vhi vlo td tr tf + <R=repeat> <)> 154 tsample data <RB=val> tsample data <RB=val> 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). HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Parameter Description 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 155 5: Sources and Stimuli Independent Source Functions Example The following b-string and its repeat time R and repeating start bit RB cannot use parameter—it is considered as a undivided unit in HSPICE and can only be defined in pattern 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: ■ High voltage is 2 V. ■ Low voltage is 0 V. ■ Time delay is 40 ps. ■ 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 pattern command, which is explained later in this section. The following general syntax is for an NS pattern source. Syntax Vxxx n+ n- PAT <(> vhi vlo td tr tf tsample + [component 1 ... component n] <RB=val> <R=repeat> <)> Ixxx n+ n- PAT <(> vhi vlo td tr tf tsample + [component 1 ... component n] <RB=val> <R=repeat> <) > 156 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 157 5: Sources and Stimuli Independent Source Functions 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 pattern-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 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 (PRBS Function) The Pseudo Random Bit Generator Source 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. 158 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Independent Source Functions Linear Feedback Shift Register 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 MSequence 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. 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). HSPICE® Simulation and Analysis User Guide X-2005.09 159 5: Sources and Stimuli Independent Source Functions 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 PRBS Syntax The Pseudo Random Bit Generator Source uses the following syntax. Syntax lxxx n+ n- LFSR <(> vlow vhigh tdelay trise tfall rate seed <[> + taps <]> <rout=val> <)> 160 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 X-2005.09 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, ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 161 5: Sources and Stimuli Voltage and Current Controlled Elements ■ The taps are [10, 5, 3, 2]. ■ The output resistance is 0 ohm. Example 3 This example shows an entire netlist, which contains one PRBS voltage source: You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/prbs.sp 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: ■ MOS transistors ■ bipolar transistors ■ tunnel diodes ■ SCRs ■ analog functions, such as: • operational amplifiers • summers • comparators • voltage-controlled oscillators • 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. 162 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage and Current Controlled Elements ■ ■ ■ ■ 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. 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 non-linear functions. See the HSPICE Applications Manual for detailed PWL examples. HSPICE® Simulation and Analysis User Guide X-2005.09 163 5: Sources and Stimuli Voltage and Current Controlled Elements 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 ) + … Parameter Description FV Controlled voltage or current, from the controlled source. 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 2.5 164 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage and Current Controlled Elements 1. 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). 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 165 5: Sources and Stimuli Voltage and Current Controlled Elements 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 ) + … 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 = 5 166 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage and Current Controlled Elements 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. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 167 5: Sources and Stimuli Power Sources 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. ■ 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. 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. 168 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Power Sources 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. 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 option=POWER_DB, then the value is in decibels; otherwise it is in Watts*POWER_SCAL. In this equation, POWER_SCAL is a scaling factor that you specify in the .OPTION statement. 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...) HSPICE® Simulation and Analysis User Guide X-2005.09 169 5: Sources and Stimuli Power Sources Parameter Description 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. 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: 170 ■ The DC impedance is 2 mega-ohms. ■ The AC impedance is 100 kilo-ohms. ■ The phase offset is 60 degrees. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Table 12 Independent Source Options Option Description POWER_SCAL Sets the scaling factor for power values. • If you specify this value, the power unit is in Watts*POWER_SCAL. • Default is 1. POWER_DB Specifies that the power value is in decibels. 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 X-2005.09 171 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Voltage-Controlled Voltage Source (VCVS) The syntax is: Linear Exxx n+ n- <VCVS> in+ in- gain <MAX=val> <MIN=val> + <SCALE=val> <TC1=val> <TC2=val><ABS=1> <IC=val> 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. 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> ... 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. Delay Element Exxx n+ n- <VCVS> DELAY in+ in- TD=val <SCALE=val> + <TC1=val> <TC2=val> <NPDELAY=val> 172 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Laplace Transform Syntax Transconductance H(s): Gxxx n+ n- LAPLACE in+ in- k0, k1, ..., kn / d0, + d1, ..., dm <SCALE=val> <TC1=val> <TC2=val> <M=val> Voltage Gain H(s): Exxx n+ n- LAPLACE in+ in- k0, k1, ..., kn / d0, + d1, ..., dm <SCALE=val> <TC1=val> <TC2=val> H(s) is a rational function, in the following form: k0 + k1 s + … + kn sn H ( s ) = --------------------------------------------------d0 + d1 s + … + dm s m You can use parameters to define the values of all coefficients (k0, k1, ..., d0, d1, ...). Example Glowpass 0 out LAPLACE in 0 Ehipass out 0 LAPLACE in 0 1.0 / 1.0 2.0 2.0 1.0 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 X-2005.09 173 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Pole-Zero Function Syntax Transconductance H(s): Gxxx n+ n- POLE in+ in- a αz1, fz1, ..., αzn, fzn / b, + αp1, fp1, ..., αpm, fpm <SCALE=val> <TC1=val> + <TC2=val> <M=val> Voltage Gain H(s): Exxx n+ n- POLE in+ in- a αz1, fz1, ..., αzn, fzn / b, + αp1, fp1, ..., αpm, fpm <SCALE=val> <TC1=val> + <TC2=val> The following equation defines H(s) in terms of poles and zeros: a ⋅ ( s + α z1 – j2 π f z1 )… ( s + α zn – j2 π f zn ) ( s + α zn + j2 π f zn ) H ( s ) = -----------------------------------------------------------------------------------------------------------------------------------------------------b ⋅ ( s + α p1 – j2 π f p1 )… ( s + α pm – j2 π f pm ) ( s + α pm + j2 π f 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. 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 + j2 π ⋅ 0.1379 ) ( s + 0.5 – ( j2 π ⋅ 0.1379 ) ) 174 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Frequency Response Table Syntax Transconductance H(s): Gxxx n+ n- FREQ in+ inf1, a1, φ1, ..., fi, ai, φ1 + <DELF=val> <MAXF=val> <SCALE=val> <TC1=val> + <TC2=val> <M=val> <LEVEL=val> <ACCURACY=val> Voltage Gain H(s): Exxx n+ n- FREQ in+ inf1, a1, φ1, ..., fi, ai, φ1 + <DELF=val> <MAXF=val> <SCALE=val> <TC1=val> + <TC2=val> <LEVEL=val> <ACCURACY=val> ■ Each fi is a frequency point, in hertz. ■ ai is the magnitude, in dB. ■ φ1 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 ( j2 π f ) = ----------------------------- ( log f – log f i ) + a i log f i – log f k φi – φk ∠H ( j2 π f ) = --------------- ( f – f i ) + φ i fi – fk 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 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 175 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements 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. Behavioral Voltage Source Syntax Exxx n+ n- VOL=’equation’ <MAX=val> <MIN=val> Ideal Op-Amp Syntax Exxx n+ n- OPAMP in+ inYou can also substitute Level=1 in place of OPAMP: Exxx n+ n- in+ in- level=1 Ideal Transformer Syntax 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 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. 176 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Parameter Description 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 177 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E 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/ min 〈 TD, tstop〉 tstep. That is, NPDELAY default = max ---------------------------------------, 10 tstep The .TRAN statement specifies tstep and tstop values. OPAMP or Level=1 The keyword for an ideal op-amp element. OPAMP is a HSPICE reserved word; do not use it as a node name. 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 164). 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 ⋅ ∆ t + TC2 ⋅ ∆ t 2 ) TD Keyword for the time (propagation) delay. TRANSFORM Keyword for an ideal transformer. TRANSFORMER is a reserved ER word; do not use it as a node name. or Level=2 VCVS 178 Keyword for a voltage-controlled voltage source. VCVS is a reserved word; do not use it as a node name. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements Parameter Description x1,... Controlling voltage across the in+ and in- nodes. The x values must be in increasing order. y1,... Corresponding element values of x. 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 k:1 .. V1 Equivalent HSPICE model I2 I1 I2 V2 <=> V1 I1=k*I2 + - V2 V1=k*V2 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. HSPICE® Simulation and Analysis User Guide X-2005.09 179 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements 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 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 1.75 180 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Voltage Sources — E Elements 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. In the following 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. 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, the 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 HSPICE® Simulation and Analysis User Guide X-2005.09 181 5: Sources and Stimuli Current-Dependent Current Sources — F Elements ■ delta_v1 is the AC voltage variation of v(1) ■ delta_v2 is the AC voltage variation of v(2) Example You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/eelm.sp The AC voltage of node n3 is: v(n3) = 1.0 *v(n1)(ac) + 1.0 * v(n2)(ac) = 1.0 * 5.0 + 1.0 * 2.0 = 7.0 (v) 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. 182 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Current-Dependent Current Sources — F Elements 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. Delay Element Fxxx n+ n- <CCCS> DELAY vn1 TD=val <SCALE=val> + <TC1=val><TC2=val> NPDELAY=val Note: G Elements with algebraics make F Elements obsolete. You can still use F Elements for backward-compatibility with existing designs. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 183 5: Sources and Stimuli Current-Dependent Current Sources — F Elements Parameter Description 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. 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 164. 184 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. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Current-Dependent Current Sources — F Elements Parameter Description TC1,TC2 First-order and second-order temperature coefficients. Temperature changes update the SCALE: SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ ∆ t + TC2 ⋅ ∆ t 2 ) 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. y1,... Corresponding output current values of x. Example 1 F1 13 5 VSENS MAX=+3 MIN=-3 5 Example 1 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. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 185 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements Example 2 F2 12 10 POLY VCC 1MA 1.3M Example 2 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). Example 3 Fd 1 0 DELAY vin TD=7ns SCALE=5 Example 3 is a delayed, current-controlled current source. Example 4 Filim 0 out PWL(1) vsrc -1a,-1a 1a,1a Example 4 is a piecewise-linear, current-controlled current source. 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) The Level=0 syntax is: 186 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements Linear Gxxx n+ n- <VCCS> in+ in- transconductance <MAX=val> + <MIN=val> <SCALE=val> <M=val> <TC1=val> <TC2=val> + <ABS=1> <IC=val> 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> 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> 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. Delay Element Gxxx n+ n- <VCCS> DELAY in+ in- TD=val <SCALE=val> + <TC1=val> <TC2=val> NPDELAY=val Laplace Transform For details, see Laplace Transform on page 173. HSPICE® Simulation and Analysis User Guide X-2005.09 187 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements Pole-Zero Function For details, see Pole-Zero Function on page 174. Frequency Response Table For details, see Frequency Response Table on page 175. Behavioral Current Source (Noise Model) Syntax Gxxx n+ n- CUR=’equation’ <MAX>=val> <MIN=val> <M=val> + <SCALE=val> * correlated noise source gname node1 node2 noise=’noise_equation’ This syntax creates a simple two-terminal current noise source, whose value is described in A/sqrt(Hz). The output noise generated from this noise source is: noise_equation*H H is the transfer function from the terminal pair (node1,node2) to the circuit output, where the output noise is measured. * correlated noise source gname node1 node2 node3 node4 noise=’noise_equation’ This syntax produces a noise source correlation between the terminal pairs (node1 node2) and (node3 node4). The resulting output noise is computed as: noise_equation*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_equation expression can involve node voltages and currents through voltage sources. 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> 188 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements 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> 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> 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> Voltage-Controlled Capacitor (VCCAP) Level=2 (NPWL) and Level=3 (PPWL) piecewise linear syntax is: 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. Use the NPWL and PPWL functions to interchange the n+ and n- nodes, but use the same transfer function. The following summarizes this action: HSPICE® Simulation and Analysis User Guide X-2005.09 189 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-). 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+). PPWL 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-). 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+). If the in- node does not connect to either n+ or n-, then HSPICE or HSPICE RF changes NPWL and PPWL to PWL. Parameter Description ABS Output is an absolute value, if ABS=1. CUR, VALUE Current output that flows from n+ to n-. The equation that you define can be a function of: • • • • • DELAY 190 node voltages branch currents time (time variable) temperature (temper variable) frequency (hertz variable) 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. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements Parameter Description 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 191 5: Sources and Stimuli Voltage-Dependent Current Sources — G 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 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 164). 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. TC1,TC2 First-order and second-order temperature coefficients. Temperature changes update the SCALE: SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ ∆ t + TC2 ⋅ ∆ t 2 ) . TD Keyword for the time (propagation) delay. transconductance Voltage-to-current conversion factor. transfactor 192 Voltage-to-resistance conversion factor. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements Parameter Description 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 193 5: Sources and Stimuli Voltage-Dependent Current Sources — G Elements 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)’ 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 194 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Current-Dependent Voltage Sources — H Elements 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 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> HSPICE® Simulation and Analysis User Guide X-2005.09 195 5: Sources and Stimuli Current-Dependent Voltage Sources — H Elements 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 Hxxx n+ n- <CCVS> DELAY vn1 TD=val <SCALE=val> <TC1=val> + <TC2=val> <NPDELAY=val> Note: E Elements with algebraics make CCVS elements obsolete. You can still use CCVS elements for backward-compatibility with existing designs. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Current-Dependent Voltage Sources — H Elements Parameter Description 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. 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〉 That is: NPDELAY default = max ---------------------------------------, 10 . tstep 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 164. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 197 5: Sources and Stimuli Current-Dependent Voltage Sources — H Elements Parameter Description SCALE Multiplier for the element value. TC1,TC2 First-order and second-order temperature coefficients. Temperature changes update the SCALE: SCALEeff = SCALE ⋅ ( 1 + TC1 ⋅ ∆ t + TC2 ⋅ ∆ t 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. H Element Examples 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 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 198 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Digital and Mixed Mode Stimuli independent voltage source, you must insert a dummy independent voltage source. Example .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: ■ FA1=VIN1 ■ FA2=VIN2 ■ P0=0 ■ P1=0 ■ P2=0 ■ P3=0 ■ P4=1 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 HSPICE Signal Integrity Guide. HSPICE® Simulation and Analysis User Guide X-2005.09 199 5: Sources and Stimuli Digital and Mixed Mode Stimuli 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 a08 ... a56 ... a01 a02 a03 a04 a05 a06 a07 \ a09 a10 a11 a12 a13 a14 a15 \ * Continuation of signal names a57 a58 a59 a60 a61 a62 a63 End of signal names Remainder of file General Form The general syntax for a U element digital source is: Uxxx interface nlo nhi mname SIGNAME = sname IS = val 200 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). HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Digital and Mixed Mode Stimuli SIGNAME= sname Signal name, as referenced in the digital output file header. Can be a string of up to eight alphanumeric characters. IS=val 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 13 Digital-to-Analog Parameters Names (Alias) Units Default Description CLO farad 0 Capacitance, to low-level node. CHI farad 0 Capacitance, to high-level node. S0NAME State 0 character abbreviation. A string of up to four alphanumerical characters. 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 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 HSPICE® Simulation and Analysis User Guide X-2005.09 State 19 character abbreviation. A string of up to four alphanumerical characters. 201 5: Sources and Stimuli Digital and Mixed Mode Stimuli Table 13 Digital-to-Analog Parameters (Continued) Names (Alias) Units Default Description 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. 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). You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/sources/uelm.sp 202 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Digital and Mixed Mode Stimuli The associated digital input file is: 1 00 09 10 11 20 30 39 40 41 50 60 70 80 1:1 z:1 0:1 z:1 1:1 0:1 x:1 1:1 x:1 0:1 1:1 0:1 1:1 U Element Digital Outputs The general syntax for a digital output in a HSPICE output (not supported in HSPICE RF) is: U<name> 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= sname 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...> Digital output (not supported in HSPICE RF). HSPICE® Simulation and Analysis User Guide X-2005.09 203 5: Sources and Stimuli Digital and Mixed Mode Stimuli Analog-to-Digital Output Model Parameters Table 14 Analog-to-Digital Parameters Name (Alias) Units Default Description RLOAD ohm 1/gmin Output resistance. CLOAD farad 0 Output capacitance. 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 1E-9 Step size for digital input file. Scale factor for time. 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. 204 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Digital and Mixed Mode Stimuli 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 X-2005.09 205 5: Sources and Stimuli Replacing Sources With Digital Inputs Replacing Sources With Digital Inputs Figure 26 Digital File Signal Correspondence Traditional voltage pulse sources ... 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 ... become D2A drivers ... 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 ... that get their input from the Digital stimulus file ... <designname>.d2a Signalname list Time (in model time units) Statechange: Signal list 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 0:1 300 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. The pathname to this example is: $installdir/demo/hspice/cchar/digin.sp * 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 206 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Replacing Sources With Digital Inputs UCO carry_out REF A2D SIGNAME=12 R1 REF 0 1k * 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=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. For another example, see the file identified below and the plot in Figure 27. $installdir/demo/hspice/cchar/tdgtl.sp In this next 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 above. HSPICE or HSPICE RF outputs a digital file. HSPICE® Simulation and Analysis User Guide X-2005.09 207 5: Sources and Stimuli Specifying a Digital Vector 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: ■ Vector Pattern Definition section ■ Waveform Characteristics section ■ Tabular Data section To incorporate this information into your simulation, include the .VEC command in your netlist. 208 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Specifying a Digital Vector File Commands in a Digital Vector File For descriptions of all commands that you can use in a VEC file, see the HSPICE Command Reference Manual. 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 209. 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. 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: HSPICE® Simulation and Analysis User Guide X-2005.09 209 5: Sources and Stimuli Specifying a Digital Vector File 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 shows the legal states for an input signal. Signal values can have any of these legal states. Table 15 Legal States for an Input Signal 210 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. L Resistive drive to ZERO (gnd). An OUT or OUTZ statement defines resistance value. HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Specifying a Digital Vector File Table 15 Legal States for an Input Signal (Continued) 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 16. Table 16 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. HSPICE® Simulation and Analysis User Guide X-2005.09 211 5: Sources and Stimuli Specifying a Digital Vector File For example, ... IO OOOO; start of tabular section data 11.0 20.0 30.0 35.0 1001 1100 1000 xx00 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> 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. 212 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Specifying a Digital Vector File 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. 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 209. 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 X-2005.09 213 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. 214 HSPICE® Simulation and Analysis User Guide X-2005.09 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 X-2005.09 215 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 statement 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. 216 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Specifying a Digital Vector File Do not specify absolute unit values in a .PARAM statement. For example, if in your netlist: .param myperiod = 10ns $ ‘ns’ makes this incorrect 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 HSPICE® Simulation and Analysis User Guide X-2005.09 217 5: Sources and Stimuli Specifying a Digital Vector File In these statements, the unit is volts. ■ 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 ... 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 218 HSPICE® Simulation and Analysis User Guide X-2005.09 5: Sources and Stimuli Specifying a Digital Vector File vih 3.3 1 0 000 vih 5.0 0 0 FFF ; to specify logic low, use ‘vil’ ;**************************************************** ; 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 X-2005.09 219 5: Sources and Stimuli Specifying a Digital Vector File 220 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions 6 Parameters and Functions 6 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 HSPICE Command Reference manual. HSPICE® Simulation and Analysis User Guide X-2005.09 221 6: Parameters and Functions Using Parameters in Simulation (.PARAM) Using Parameters in Simulation (.PARAM) Defining Parameters Parameters in HSPICE are names that you associate with numeric values. (See “Defining Parameters.”) You can use any of these methods to define parameters: Table 17 .PARAM 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 226. 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 222 .PARAM <mcVar> = Agauss(1.0,0.1) HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Using Parameters in Simulation (.PARAM) Table 17 .PARAM Syntax (Continued) Parameter Description .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 268) .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 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. Parameter resolution order is: 1. Resolve all literal assignments. 2. Resolve all expressions. 3. Resolve all function calls. Table 18 shows the parameter passing order. Table 18 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) HSPICE® Simulation and Analysis User Guide X-2005.09 223 6: Parameters and Functions Using Parameters in Simulation (.PARAM) 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. The parameter keeps the assigned value, unless: ■ Later definition changes its value, or ■ Algebraic expression assigns a new value during simulation. HSPICE does not warn you, if they reassign 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 about simulation output.) Example .PRINT DC v(3) gain = PAR(‘v(3)/v(2)’) PAR(‘v(4)/v(2)’) 224 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Using Parameters in Simulation (.PARAM) 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. The format of a function is: funcname1(arg1[,arg2...]) = expression1 + [funcname2(arg1[,arg2...]) = expression2] off ■ 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. 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. off Voids all user-defined functions. Example 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 HSPICE® Simulation and Analysis User Guide X-2005.09 225 6: Parameters and Functions Using Algebraic Expressions a .PARAM statement. For a description of the .MEASURE statement, see Specifying User-Defined Analysis (.MEASURE) on page 268. .PRINT|.PROBE|.PLOT|.GRAPH Parameters .PRINT|.PROBE|.PLOT|.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|.GRAPH statement, not in a .PARAM statement. HSPICE RF does not support .PLOT|.GRAPH statements. For more information about the .PRINT|.PROBE|.PLOT|.GRAPH statements, see Displaying Simulation Results on page 244. 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 64. 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’ 226 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Built-In Functions and Variables 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.) Built-In Functions and Variables In addition to simple arithmetic operations (+, -, *, /), HSPICE provides several built-in functions and variables, listed in Table 19 and Table 20 respectively, that you can use in expressions: Table 19 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) HSPICE® Simulation and Analysis User Guide X-2005.09 227 6: Parameters and Functions Built-In Functions and Variables Table 19 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function Class Description 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 x**y power 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 228 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Built-In Functions and Variables Table 19 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function Class Description 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 args control Returns the numeric maximum of x and y val(element) get value various Returns a parameter value for a specified element. For example, val(r1) returns the resistance value of the r1 resistor. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 229 6: Parameters and Functions Built-In Functions and Variables Table 19 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function Class Description lv (<Element>) or lx (<Element>) element templates various Returns various element values during simulation. See Element Template Output on page 267 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. .param z=’condition ? x: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. 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. .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) .para x=y>=z (y greater than or equal to z) .para x=y==z (y equal to z) 230 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Built-In Functions and Variables Table 19 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function Class Description 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 20 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 20 Synopsys HSPICE Special Variables HSPICE Form time Function Class Description current simulation time control Uses parameters to define the current simulation time, during transient analysis. HSPICE® Simulation and Analysis User Guide X-2005.09 231 6: Parameters and Functions Parameter Scoping and Passing Table 20 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. 232 HSPICE® Simulation and Analysis User Guide X-2005.09 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 sub-circuits 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. HSPICE® Simulation and Analysis User Guide X-2005.09 233 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. 234 HSPICE® Simulation and Analysis User Guide X-2005.09 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 21 compares the three primary methods for configuring libraries, to achieve required parameter checking for default MOS transistor widths. Table 21 Method Local Methods for Configuring Libraries Parameter Location On a .SUBCKT definition line Pros Cons 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. HSPICE® Simulation and Analysis User Guide X-2005.09 235 6: Parameters and Functions Parameter Scoping and Passing Table 21 Method Methods for Configuring Libraries (Continued) Parameter Location Pros Cons 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. Special .OPTION DEFW statement 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 236 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Parameter Scoping and Passing 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 ■ 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, which uses the same scoping rules that HSPICE used before Release 95.1. Example This example explicitly shows the difference between local and global scoping for using parameters in sub-circuits. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 237 6: Parameters and Functions Parameter Scoping and Passing .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 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 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. 238 HSPICE® Simulation and Analysis User Guide X-2005.09 6: Parameters and Functions Parameter Scoping and Passing Figure 28 + Hierarchical Parameter Passing Problem Sub1 Sub2 Sub3 r1 r2 r3 1V - 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 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 22, based on how you set .OPTION PARHIER to local/global: Table 22 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 HSPICE® Simulation and Analysis User Guide X-2005.09 239 6: Parameters and Functions Parameter Scoping and Passing 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 X-2005.09 7: Simulation Output Overview of Output Statements 7 Simulation Output 7 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 Manual. Overview of Output Statements Output Commands The input netlist file contains output statements, including .PRINT, .PLOT, .GRAPH, .PROBE, .MEASURE, and .DOUT. 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 AvanWaves interface files. HSPICE® Simulation and Analysis User Guide X-2005.09 241 7: Simulation Output Overview of Output Statements HSPICE RF supports only .OPTION POST, .OPTION PROBE, .PRINT, .PROBE, and .MEASURE. It does not support .DOUT, .PLOT, .GRAPH, or .STIM. AvanWaves provides high-resolution, post-simulation, and interactive display of waveforms. Table 23 Output Statements Output Statement Description .PRINT Prints numeric analysis results in the output listing file (and postprocessor data, if you specify .OPTION POST). .PLOT 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). (HSPICE only) .GRAPH (HSPICE only) 242 Obsolete option. Use .PRINT or ..PROBE to generate necessary plot in the output listing file. Generates highresolution plots for specific printing devices (such as HP LaserJet), or in PostScript format (intended for hard-copy outputs, without using a post-processor). .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 Specifies simulation results to transform to PWL, Data Card, or Digital Vector File format. Not supported in HSPICE RF. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Overview of Output Statements 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: ■ DC and transient analysis ■ AC analysis ■ element template (HSPICE only; not supported in HSPICE RF) ■ .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. This analysis is available in HSPICE only; HSPICE RF does not support element template output. 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 226 or HSPICE RF. HSPICE® Simulation and Analysis User Guide X-2005.09 243 7: Simulation Output Displaying Simulation Results 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) 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 netlist, before the .PRINT statement. 244 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Displaying Simulation Results .PLOT Statement Note: This is an obsolete statement. You can gain the same functionality by using the .PRINT Statement. The .PLOT statement plots the output values of one or more variables, in a selected HSPICE analysis. Each .PLOT statement defines the contents of one plot, which can contain more than one output variable. Note: You cannot use .PLOT in HSPICE RF. If you do not specify plot limits, HSPICE determines the minimum and maximum values of each output variable that it plots, and scales each plot to fit common limits. To force HSPICE to set limits for certain variables, set the plot limits to (0,0) for the variables. 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 to 80, the plot has 50 columns. If CO is 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. HSPICE® Simulation and Analysis User Guide X-2005.09 245 7: Simulation Output Displaying Simulation Results .GRAPH Statement Note: This is an obsolete statement. You can gain the same functionality by using the .PROBE Statement. 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 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 HSPICE Command Reference manual. HSPICE RF does not support the .GRAPH statement. Table 24 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 “Modeling Filters and Networks” in the HSPICE Applications Manual). XGRID , YGRID 246 0.0 Set these values to 1.0, to turn on the axis grid lines. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Displaying Simulation Results Table 24 Model Parameters (Continued) Name (Alias) Default Description XMIN, XMAX 0.0 • 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. XSCA L 1.0 Scale for the x-axis. Two common axis scales are: YMIN, YMAX 0.0 Linear(LIN) (XSCAL = 1) Logarithm(LOG) (XSCAL = 2) If YMIN is not equal to YMAX, then YMIN and YMAX determine the yaxis 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. YSCA L 1.0 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(*) HSPICE® Simulation and Analysis User Guide X-2005.09 247 7: Simulation Output Displaying Simulation Results ***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 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 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*). 248 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Displaying Simulation Results Print Control Options The codes that you can use to specify the element templates for output in HSPICE or HSPICE RF are: ■ .OPTION CO to set column widths in printouts. ■ .WIDTH statement to set the width of a printout. ■ .OPTION INGOLD for output in exponential form. ■ .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. HSPICE® Simulation and Analysis User Guide X-2005.09 249 7: Simulation Output Displaying Simulation Results 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 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 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters 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. 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; HSPICE RF does not support element template output). For each device type, the templates contain: • values of variables that you set • state variables • element charges • capacitance currents HSPICE® Simulation and Analysis User Guide X-2005.09 251 7: Simulation Output Selecting Simulation Output Parameters • capacitances • derivatives Print Control Options on page 249 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. 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) 252 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). HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters Example .PLOT TRAN I(VIN) .PRINT DC I(X1.VSRC) .PLOT DC I(XSUB.XSUBSUB.VY) Current: Element Branches Syntax In(Wwww) Iall(Wwww) 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. HSPICE® Simulation and Analysis User Guide X-2005.09 253 7: Simulation Output Selecting Simulation Output Parameters 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. 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) I1 (R1) node1 R1 I2 (R1) Figure 30 node2 Inductor (node1, node2); capacitor (node 1, node2) node1 I1(L1) I1(C1) I2(L1) I2(C1) node2 254 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters Figure 31 Figure 32 Diode (node1, node2) I1 (D1) node1 (anode, P-type, + node) I2 (D2) node2 (anode, N-type, - node) 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) HSPICE® Simulation and Analysis User Guide X-2005.09 255 7: Simulation Output Selecting Simulation Output Parameters 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) 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. 256 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters 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). 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 X-2005.09 257 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' ÞIstot ■ Lateral Pd = Vc'e' ⋅ Ico + Vb'e' ⋅ Ibo + Vcc' ⋅ Ictot + Vbb' ⋅ Ibtot + Vee' ⋅ Ietot + Vsb' ⋅ Iso – Vbb' ÞIstot 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 X-2005.09 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 X-2005.09 259 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 25 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 X-2005.09 7: Simulation Output Selecting Simulation Output Parameters Table 25 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) HSPICE® Simulation and Analysis User Guide X-2005.09 261 7: Simulation Output Selecting Simulation Output Parameters Nodal Voltage Syntax Vz(n1<,n2>) Parameter Description z Specifies the voltage output type (see Table 25 on page 261) n1, n2 Specifies node names. If you omit n2, HSPICE or HSPICE RF assumes ground (node 0). Example .PLOT AC VM(5) VDB(5) VP(5) The preceding 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. 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. ■ Real and imaginary: VR(N1,N2) = VI(N1,N2) = 262 REAL [V(N1,0)] - REAL [V(N2,0)] IMAG [V(N1,0)] - IMAG [V(N2,0)] HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters ■ 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)) SPICE Method Example: ■ Real and imaginary: VR(N1,N2) = REAL [V(N1,0) - V(N2,0)] VI(N1,N2) = IMAG [V(N1,0) - V(N2,0)] ■ Magnitude: VM(N1,N2) = [VR(N1,N2)2+VI(N1,N2)2]0.5 ■ Phase: VP(N1,N2) = ARCTAN[VI(N1,N2)/VR(N1,N2)] ■ Decibel: VDB(N1,N2) = 20 ⋅ LOG10[VM(N1,N2)] Current: Independent Voltage Sources Syntax Iz(Vxxx) Parameter Description z Current output type (see Table 25 on page 261). 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, IM(X1.Vxxx). HSPICE® Simulation and Analysis User Guide X-2005.09 263 7: Simulation Output Selecting Simulation Output Parameters Example .PLOT AC IR(V1) IM(VN2B) IP(X1.X2.VSRC) This example applies to HSPICE, but not to HSPICE RF. Current: Element Branches Syntax Izn(Wwww) Parameter Description z Current output type (see Table 25 on page 261). 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) 264 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 265 7: Simulation Output Selecting Simulation Output Parameters Parameter Description z Output type (see Table 25 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. Noise and Distortion This section describes the variables used for noise and distortion analysis. Syntax ovar <(z)> 266 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. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Selecting Simulation Output Parameters 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 .PRINT, .PROBE (HSPICE and HSPICE RF), .PLOT, and .GRAPH (HSPICE only) 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 HSPICE RF does not support element template output. 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) HSPICE® Simulation and Analysis User Guide X-2005.09 267 7: Simulation Output Specifying User-Defined Analysis (.MEASURE) 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. See the HSPICE Command Reference manual for more information about the INTERP option. Fundamental measurement modes in HSPICE are: 268 ■ Rise, fall, and delay ■ Find-when ■ Equation evaluation ■ Average, RMS, min, max, and peak-to-peak ■ Integral evaluation ■ Derivative evaluation ■ Relative error HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Specifying User-Defined Analysis (.MEASURE) 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. See the HSPICE Command Reference manual for information about .OPTION MEASFAIL. 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. See the HSPICE Command Reference manual for more information. In versions of HSPICE before 2003.09, to automatically sort large numbers of .MEASURE statements, you could use the .OPTION MEASSORT statement. 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) 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 HSPICE® Simulation and Analysis User Guide X-2005.09 269 7: Simulation Output Specifying User-Defined Analysis (.MEASURE) 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: .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. 270 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Specifying User-Defined Analysis (.MEASURE) 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 244. 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 271 7: Simulation Output Specifying User-Defined Analysis (.MEASURE) ■ 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’ 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. 272 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Specifying User-Defined Analysis (.MEASURE) 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 ERR1 i = --------------------------------------------- , i = 1,NPTS max (MINVAL,M i) 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) HSPICE® Simulation and Analysis User Guide X-2005.09 273 7: Simulation Output .SURGE Statement 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. .SURGE Statement The .SURGE statement in HSPICE RF automatically detects and reports a current surge that exceeds the specified surge tolerance. Surge current is the current flowing into or out of a node to the lower sub-circuit hierarchy. HSPICE does not use the .SURGE statement. Syntax .SURGE surge_threshold surge_width node1 < node2 .... noden > Parameter Description surge_threshold Defines the minimum absolute surge current. surge_width Defines the minimum duration of a surge. nodex Can be any valid node name, at the current or lower subcircuit level. The .SURGE statement reports any current surge that is greater than surge_threshold for a duration of more than surge_width. 274 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output .CHECK Statements Example In the example below, the .SURGE statement detects any current surge that has an absolute amplitude of more than 1mA, and that exceeds 100ns, x(xm.x1.a), x(xm.x2.c), and x(xn.y). .SUBCKT sa a b ... .ENDS .SUBCKT sb c d ... .ENDS .SUBCKT sx x y x1 x y sa x2 x a sb .ENDS xm 1 2 sx xn 2 a sx .SURGE 1mA 100ns xm.x1.a xm.x2.c xn.y .CHECK Statements The .CHECK statements in HSPICE RF offer the following instrumentation: ■ Setting Global Hi/Lo Levels ■ Slew, Rise, and Fall Conditions ■ Edge Timing Verification ■ Setup and Hold Verification ■ IR Drop Detection The results of these statements appear in a file with an .err filename extension. To prevent creating unwieldy files, HSPICE RF reports only the first 10 violations for a particular check, in the .err file. Note: HSPICE does not support the .CHECK statement. Setting Global Hi/Lo Levels To globally set the desired high and low definitions for all .CHECK statements, use the GLOBAL_LEVEL command. HSPICE® Simulation and Analysis User Guide X-2005.09 275 7: Simulation Output .CHECK Statements Syntax .CHECK GLOBAL_LEVEL (hi lo hi_th lo_th) Parameter Description hi Value for logic high. lo Value for logic low. hi_th Is the minimum value considered high. lo_th Is the maximum value considered low. These parameters can be either numbers or expressions, and hi_th and lo_th can be either absolute values or percentages, if punctuated with the % symbol. You can also locally set different logic levels for individual timing checks. Example The first example defines a logic high as 5 volts, and a logic low as 0 volts. A voltage value as small as 4 volts is considered high, while a value up to 1 volt is low. .CHECK GLOBAL_LEVEL (5 0 4 1) The second example illustrates an alternative definition for the first example: .CHECK GLOBAL_LEVEL (5 0 80% 20%) Slew, Rise, and Fall Conditions 276 ■ To verify that a slew rate occurs within the specified window of time, use the CHECK SLEW command. ■ To verify that a rise time occurs within the specified window of time, use the CHECK RISE command. ■ To verify that a fall time occurs within the specified window of time, use the CHECK FALL command. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output .CHECK Statements Syntax .CHECK SLEW (min <(hi lo hi_th .CHECK RISE (min <(hi lo hi_th .CHECK FALL (min <(hi lo hi_th max) node1 <node2 ...> lo_th)> max) node1 <node2 ...> lo_th)> max) node1 <node2 ...> lo_th)> Parameter Description min Is the lower boundary for the time window. max Is the upper limit. node1 < node2 ... > Is a list of all nodes to check. Note: When you specify node names, you can use the wildcard character (*). You can also use the hi, lo, hi_th, and lo_th parameters to set local logic levels for each particular timing check. Example This example defines a window between 1.5 and 2.2 nanoseconds (ns) wide, in which the va and vb signals must complete their rise transition. Values for hi, lo, and the thresholds are defined in .CHECK GLOBAL_LEVEL, which is described in the section Setting Global Hi/Lo Levels on page 275. .CHECK RISE (1.5ns 2.2ns) va vb Figure 35 illustrates this example. Figure 35 RISE Time Example HI HI_thresh LO_thresh LO 1.5 ns < t < 2.2 ns HSPICE® Simulation and Analysis User Guide X-2005.09 277 7: Simulation Output .CHECK Statements The next example sets the condition that a* nodes must have a slew rate between (HI_thresh - LO_thresh)/3ns and (HI_thresh - LO_thresh)/1ns. If either node has a slew rate greater than that defined in the .CHECK SLEW statement, HSPICE RF reports the violation in the .err file. .CHECK SLEW (1ns 3ns) a* (3.3 0 2.6 0.7) The slew rate check in Figure 36 defines its own hi, lo, and corresponding threshold values, as indicated by the four values after the node names. Figure 36 SLEW Example 3.3 2.6 0.7 0.0 1ns < t < 3ns Edge Timing Verification The edge condition verifies that a triggering event provokes an appropriate RISE or FALL action, within the specified time window. Syntax .CHECK EDGE (ref RISE|FALL min max RISE|FALL) + node1 < node2 ... > < (hi lo hi_th low_th) > Parameter Description ref Name of the reference signal. min Minimum time. max Maximum time. node1 < node2 ... > List of nodes to which you apply the edge condition. You can also use the hi, lo, hi_th, and lo_th parameters to set local logic levels for each particular timing check. 278 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output .CHECK Statements Example This example sets the condition that the rising action of the clock (clk) triggers the falling edge of VOUTA within 1 to 3 ns, as shown in Figure 37: .CHECK EDGE (clk RISE 1ns 3ns FALL) VOUTA Values for hi, lo, and the thresholds are those defined in .CHECK GLOBAL_LEVEL, which is described in the section Setting Global Hi/Lo Levels on page 275. Figure 37 EDGE Example voutA CLK HI HI_thresh LO_thresh LO 1ns < t < 3 ns Setup and Hold Verification Use the SETUP and HOLD statements to ensure that specified signals do not switch for a specified period of time. Syntax .CHECK SETUP (ref RISE|FALL duration RISE|FALL) node1 \ + < node2 ... > < (hi lo hi_th low_th) > .CHECK HOLD (ref RISE|FALL duration RISE|FALL) node1 \ + < node2 ... > < (hi lo hi_th low_th) > Parameter Description ref Reference or trigger signal. node1 < node2 ... > Specified nodes for which the SETUP or HOLD condition applies. For HOLD, duration is the minimum time required after the triggering event, before the specified nodes can rise or fall. HSPICE® Simulation and Analysis User Guide X-2005.09 279 7: Simulation Output .CHECK Statements For SETUP, duration is the minimum time before the triggering event, during which the specified nodes cannot rise or fall. Example This example specifies that v1 and v2 must not switch for 2 ns, before every rising edge of nodeA. .CHECK SETUP (nodeA RISE 2ns FALL) v1 v2 Figure 38 SETUP Example nodeA v1 HI HI_thresh LO_thresh LO t > = 2ns The following example specifies that vin* (such as vin1, vin2, and so on), must not switch for 2 ns, after every falling edge of nodeA. .CHECK HOLD (nodeA FALL 2ns RISE) vin* Figure 39 HOLD Example vin* nodeA HI HI_thresh LO_thresh LO t > = 2ns 280 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output .CHECK Statements IR Drop Detection You can check that the IR drop does not exceed, or does not fall below, a specified value for a specified duration. Syntax .CHECK IRDROP ( volt_val time ) node1 < node2 ... > \ + < ( hi lo hi_th low_th ) > Parameter Description volt_val Is the limiting voltage value. • A positive volt_val (voltage value) indicates ground bounce checking. • A negative volt_val denotes VDD drop. duration Is the maximum allowable time. If you set duration to 0, then HSPICE RF reports every glitch that strays beyond the specified volt_val. node1 < node2 ... > Are the specified nodes for which the IR drop checking applies. Example The example below specifies that v1 must not fall below -2 volts for any duration exceeding 1 ns. .CHECK IRDROP (-2 1ns) v1 Figure 40 IR Drop Example v1 -2 volts t < = 1ns HSPICE® Simulation and Analysis User Guide X-2005.09 281 7: Simulation Output DSPF Flow DSPF Flow DSPF (Detailed Standard Parasitic Format) is a standard output format for parasitic extraction tools, such as Star-RC. HSPICE RF can output simulation results in this format; HSPICE does not support this format. This section provides an overview of DSPF, describes how HSPICE RF uses a DSPF file, introduces Selective DSPF Expansion, and details Multi-Threshold Selective DSPF Expansion. Note: HSPICE RF requires both a DSPF file and an ideal netlist. Very large circuits generate very large DSPF files; this is when using one of the two options described below can really improve performance. To run the simulation, using DSPF expansion, include a SIM_DSPF option in your ideal netlist. For example: .OPTION SIM_DSPF = “add4.dspf” This option maps parasitics of the DSPF file, into the hierarchical ideal netlist. Example $ models .MODEL p pmos .MODEL n nmos .INCLUDE add4.dspf .OPTION SIM_DSPF=“add4.dspf” .VEC “dspf_adder.vec” .TRAN 1n 5u vdd vdd 0 3.3 .OPTION POST .END The SIM_DSPF option accelerates the simulation by more than 100%. Using the SIM_LA option at the same time, further reduces the total CPU time: 282 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output DSPF Flow $ models .MODEL p pmos .MODEL n nmos .INCLUDE add4.dspf .OPTION SIM_DSPF=“add4.dspf” .OPTION SIM_LA=PACT .VEC “dspf_adder.vec” .TRAN 1n 5u vdd vdd 0 3.3 .OPTION POST .END To expand only active nodes, such as those that move, include the SIM_DSPF_ACTIVE option in your netlist. For example: .OPTION SIM_DSPF_ACTIVE = “active_net_filename” This option is most effective when used with a large design—for example, over 5K transistors. Smaller designs lose some of the performance gain, due to internal overhead processing. When you have included the appropriate control option, run HSPICE RF, using the ideal netlist. The structure of a DSPF file is: *|DSPF 1.0 *|DESIGN “demo” *|Date “October 6, 1998” ... .SUBCKT < name > < pins > * Net Section C1 ... R1 ... ... * Instance Section ... .ENDS Note: HSPICE RF supports only flat DSPF files; it ignores any hierarchy statements, such as .SUBCKT and .x1. HSPICE® Simulation and Analysis User Guide X-2005.09 283 7: Simulation Output DSPF Flow How HSPICE RF Uses a DSPF File HSPICE RF requires both a DSPF file, and an ideal extracted netlist. DSPF includes both a standard and a selective DSPF expansion flow. To run simulation, using the standard DSPF expansion, include an .OPTION SIM_DSPF statement in your netlist. Example .OPTION SIM_DSPF = “dspf_filename” Figure 41 ideal.in Generate DSPF Flow parser DSPF parser simulation DSPF HSPICE RF expands all nets from the DSPF file unless a selective DSPF mode is specified, in which case, see Figure 42. Note: When you use this option, you can include multiple DSPF files. SIM_DSPF_SCALER/SIM_DSPF_SCALEC These options are supported to scale the resistance and the capacitance values in the standard parasitic file for DSPF flow. Syntax .OPTION SIM_DSPF_SCALER = scaleR .OPTION SIM_DSPF_SCALEC = scaleC 284 ■ scaleR is the scale factor for resistances. ■ scaleC is the scale factor for capacitances. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output DSPF Flow Selective DSPF Expansion To invoke selective DSPF expansion, use the SIM_DSPF_ACTIVE option in your HSPICE RF netlist. HSPICE does not support the DSPF format. Syntax .OPTION SIM_DSPF_ACTIVE = “active_net_filename” If the active_net_filename file does not exist in the first run, no nets are expanded. Active nets are added to the file as they are identified in the subsequent transient simulation. A second run using the same file and option causes only the nets listed in the active_net_filename file to be expanded. It is possible that activity changes are due to timing changes caused by expansion of the active nets. In this case, additional nets are listed in the active_net_filename file and a warning is issued. By default, a node is considered active if the voltage varies by more than 0.1 V. You may change this value with the SIM_DSPF_VTOL option, described under Multi-Threshold Selective DSPF Expansion on page 286. HSPICE RF uses the active_net_filename file and the DSPF file, with the ideal netlist, to expand only the active portions of the circuit. If a net is latent, then HSPICE RF does not expand it, which saves memory and CPU time. Figure 42 on page 286 shows the selective DSPF flow. Another option available for selective DSPF expansion is SIM_DSPF_MAX_ITER. Alternate Syntax .OPTION SIM_DSPF_MAX_ITER = value Default value = 1 In this syntax, value is the number of runs for the second pass. HSPICE® Simulation and Analysis User Guide X-2005.09 285 7: Simulation Output DSPF Flow Figure 42 Selective DSPF Flow ideal.in parse active_node file exists? No simulation create active_node file Yes DSPF parses only “active” nodes simulation update (add) active_node file Multi-Threshold Selective DSPF Expansion For greater accuracy, you can specify multiple DSPF active thresholds. Syntax .OPTION SIM_DSPF_VTOL = “value | scope1 scope2 ... scopen >” In this syntax, value is the tolerance of voltage change and scopex can be a subcircuit definition, which uses a prefix of @, or a subcircuit instance. Example The value should be relatively small, compared to the operating range of the circuit, or smaller than SIM_V_SUPPLY. The first example sets the sensitivity voltage to 0.01V. Subcircuit definition snsamp and the subcircuit instance xvco have full parasitics, if their nodes move more than 0.01V during active nodes generation. xand and xff are less sensitive than the default, indicating that they are not sensitive to parasitics. .OPTION SIM_DSPF_VTOL = “0.01 | @snsamp xvco” .OPTION SIM_DSPF_VTOL = “0.25 | xand xff” 286 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Reusing Simulation Output as Input Stimuli Sample DSPF Flow Figure 43 shows a sample verification flow that includes DSPF. Figure 43 Verification Flow HSPICE RF extracted netlist (spf) Ideal Netlist HSPICE RF DSPF flow *.wdb active nets files 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. HSPICE® Simulation and Analysis User Guide X-2005.09 287 7: Simulation Output Reusing Simulation Output as Input Stimuli One .STIM statement produces one corresponding output file. Output Files The .STIM statement generates the following output files: 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. 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#. 288 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Reusing Simulation Output as Input Stimuli .POWER Statement The .POWER statement in HSPICE RF creates a table, which by default contains these measurements for every signal specified: ■ AVG ■ RMS ■ MAX ■ MIN By default, the scope of this measurement is set from zero, to the maximum time point specified in the .TRAN statement. Note: HSPICE does not support this statement. Syntax .POWER <signals> <REF = vname FROM = start_time + TO = end_time> Example .power x1.in .tran 4ps 100ps In this example, no simulation start and stop time is specified for the x1.in signal, so the simulation scope for this signal runs from the start (0ps) to the last .tran time (100ps). You can use the FROM and TO times to specify a separate measurement start and stop time for each signal: .param myendtime=80ps .power x2.in REF = a123 from=20ps to=80ps .power x0.in REF = abc from=30ps to=’myendtime - 10ps’ In this example: ■ The scope for simulating the x2.in signal is from 20 ps to 80 ps. ■ The scope for simulating the x0.in signal is from 30 ps to 70 ps. HSPICE® Simulation and Analysis User Guide X-2005.09 289 7: Simulation Output Reusing Simulation Output as Input Stimuli SIM_POWERSTART and SIM_POWERSTOP Options You can also use the SIM_POWERSTART and SIM_POWERSTOP options with the .POWER statement, to specify default start and stop times for measuring signals during simulation. These default times apply to all signals that do not have their own defined FROM and TO measurement times. Syntax .OPTION SIM_POWERSTART = < time > .OPTION SIM_POWERSTOP = < time > These options control the power measurement scope; the default is for the entire run. Example .OPTION SIM_POWERSTART = 10ps .OPTION SIM_POWERSTOP = 90ps .power x1.in In this example, the scope for simulating the x1.in signal is from 10 picoseconds (ps) to 90 ps. SIM_POWERPOST Option Syntax .OPTION SIM_POWERPOST = ON|OFF Considering the potentially enormous number of signals, there will be no waveform dumping by default for the signals in the .POWER statement. Setting SIM_POWERPOST to ON turns on power analysis. POWER_TOP Option Syntax POWER_TOP = < value > By default, power analysis is performed on the top levels of hierarchy. By applying the POWER_TOP option, you can control the number of hierarchy levels for power analysis. 290 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Reusing Simulation Output as Input Stimuli Example In the example below, HSPICE RF produces .POWER statement results for top-level and first-level subcircuits, that is, the children subcircuits of the toplevel subcircuits. .OPTION POWER_TOP = 2 POWER_ANALYSIS Option When using the POWER_ANALYSIS option, HSPICE RF traverses down all hierarchies and prints node(s) specified in the .POWER statement with larger port current than threshold current. Syntax .OPTION POWER_ANALYSIS = “< time point > < tol >” .OPTION POWER_ANALYSIS = “bottom < time point > < tol >” These two options do not return tabulated data, but do provide a list of signals that match the tolerance setting. The first POWER_ANALYSIS option produces a list of signals that consume more current than tol at time point, in this format: *** time = < time point > threshold = < tol > *** VDD = value X13.VDD = value X13.X1.VDD = value X14.VDD = value X14.X1.VDD = value The second POWER_ANALYSIS option produces the list of lowest-level signals, known as leaf subcircuits, that consume more than tol at time point. Output is similar to this: *** time = < time point > threshold = < tol > *** X13.X1.VDD = value X14.X1.VDD = value Example The POWER_ANALYSIS and .POWER statements print the names of leaf subcircuits that use more than 100uA at 100ns into the simulation into the output format. .OPTION POWER_ANALYSIS = “ bottom 100ns 100ua ” .POWER VDD HSPICE® Simulation and Analysis User Guide X-2005.09 291 7: Simulation Output Reusing Simulation Output as Input Stimuli Output Format Power analysis, using the .POWER statement, creates a table that can be read by any spreadsheet to post-process the data. Table 26 Port Name .POWER Table Header Sig# Definition Parent DepthUp DepthDn Max (A) Min (A) RMS (A) Avg (A) Tabulated data increases your analysis capability; based on the data generated in this format, you could analyze: ■ Sub-circuits that consume maximum amount of power. ■ Leaf-nodes that consume maximum amount of power. ■ Parent’s power To derive the MAX sub-block, use Depth-Up as primary key, and Avg(A) as secondary key, when sorting data. Table 27 .POWER Output Example 1 Port Name Sig# Definition Parent DepthUp DepthDn Max (A) Min (A) RMS (A) Avg (A) vdd 2 “” -1 0 2 .. .. .. 9 xa.vdd 6 “buf” 2 1 1 .. .. .. 5 xb.vdd 14 “inv” 2 1 0 .. .. .. 4 xa.x2.v dd 10 “inv” 6 2 0 .. .. .. 3 xa.x1.v dd 8 “inv” 6 2 0 .. .. .. 2 292 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Reusing Simulation Output as Input Stimuli Example The MAX leaf node could be derived by sorting data, using Depth-Dn as primary key, and Avg(A) as secondary key. Table 28 .POWER Output Example 2 Port Name Sig# Definition Parent DepthUp DepthDn Max (A) Min (A) RMS (A) Avg (A) xb.vdd 14 “inv” 2 1 0 .. .. .. 4 xa.x2.v dd 10 “inv” 6 2 0 .. .. .. 3 xa.x1.v dd 8 “inv” 6 2 0 .. .. .. 2 xa.vdd 6 “buf” 2 1 1 .. .. .. 5 vdd 2 “” -1 0 2 .. .. .. 9 To find the Parent’s power, search the corresponding parent’s ID. For example, xa.x2.vdd has a parent ID of 6: find the signal with ID 6 that consumes 5 units of average power Table 29 .POWER Output Example 3 Port Name Sig# Definition Parent DepthUp DepthDn Max (A) Min (A) RMS (A) Avg (A) xb.vdd 14 “inv” 2 1 0 .. .. .. 4 xa.x2.v dd 10 “inv” 6 2 0 .. .. .. 3 xa.x1.v dd 8 “inv” 6 2 0 .. .. .. 2 xa.vdd 6 “buf” 2 1 1 .. .. .. 5 vdd 2 “” -1 0 2 .. .. .. 9 HSPICE® Simulation and Analysis User Guide X-2005.09 293 7: Simulation Output .POWERDC Statement .POWERDC Statement The .POWERDC (standby current) statement calculates the DC leakage current in the design hierarchy. It creates a table that lists the measurements of the AVG, MAX, and MIN values for the current of every instance in the subcircuit. This table also specifies the sum of the power of each port in the subcircuit. Note: HSPICE RF supports .POWERDC only in HSPICE mode. Syntax .POWERDC <keyword> <subckt_name1...> ■ keyword is either of the following: • TOP prints the power of all the top level instances. • ALL prints the power of all the instances. Note: If you do not specify a keyword, the default is ALL. ■ subckt_name# prints the power of all instances in this subcircuit definition. Note: You can use wildcards in the subcircuit definitions. To increase the accuracy of operating point (OP) calculations, set: .opt sim_powerdc_hspice For even higher accuracy in OP calculations, set: .opt sim_powerdc_accuracy=value This sim_powerdc_accuracy setting has the same effect as the accuracy setting for transient analysis. A higher value means greater accuracy, but more time before the calculation completes. 294 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output .POWERDC Statement Output Format *** Leakage Current Result *** Subckt Name = XXX Instance Name Port Max(A) Min(A) Avg(A) ..... Total Power Max(W) Min(W) Avg(W) NOTE: Power = Sum{Ii * Vi} Subckt Name = XXX Instance Name Port Max(A) Min(A) Avg(A) ..... Total Power Max(W) Min(W) Avg(W) Example .global vdd vss .powerdc all x1 in1 mid1 inv x2 mid1 out1 inv .subckt inv in out mn out in vss vss nch mp vdd in out vdd pch .ends .end (Output) *** Leakage Current Result *** Subckt Name = Top Level Instance Name Port Max(A) x1 in ....... x1 out ....... x2 in ....... x2 out ....... Total Power ....... Subckt Name = inv Instance Name Port Max(A) mn d ....... mn g ....... mn s ....... mn b ....... mp d ....... mp g ....... mp s ....... mp b ....... Total Power ....... HSPICE® Simulation and Analysis User Guide X-2005.09 Min(A) Avg(A) Min(A) Avg(A) 295 7: Simulation Output Element Template Listings Element Template Listings This section applies only to HSPICE. HSPICE RF does not support element template output. HSPICE RF Output File Format Table 30 Resistor 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 31 Capacitor Name Alias Description CEFF LV1 Computed effective capacitance. IC LV2 Initial condition. 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 32 Inductor 296 Name Alias Description LEFF LV1 Computed effective inductance. IC LV2 Initial condition. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Table 32 Inductor (Continued) Name Alias Description 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 33 Mutual Inductor Name Alias Description K LV1 Mutual inductance. Table 34 Voltage-Controlled Current Source (G Element) Name Alias Description CURR LX0 Current, through the source, if VCCS. R LX0 Resistance value, if VCR. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 297 7: Simulation Output Element Template Listings Table 35 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 36 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. Table 37 Current-Controlled Voltage Source (H Element) 298 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. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Table 38 Independent Voltage Source Name Alias Description VOLT LV1 DC/transient voltage. VOLTM LV2 AC voltage magnitude. VOLTP LV3 AC voltage phase. Table 39 Independent Current Source Name Alias Description CURR LV1 DC/transient current. CURRM LV2 AC current magnitude. CURRP LV3 AC current phase. Table 40 Diode Name Alias Description AREA LV1 Diode area factor. AREAX LV23 Area, after scaling. IC LV2 Initial voltage, across diode. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 299 7: Simulation Output Element Template Listings Table 40 Diode (Continued) Name Alias Description C LX5 Total diode capacitance. PID LX7 Photo current, in diode. Table 41 BJT 300 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Table 41 BJT (Continued) Name Alias Description 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). 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). HSPICE® Simulation and Analysis User Guide X-2005.09 301 7: Simulation Output Element Template Listings Table 41 BJT (Continued) Name Alias Description – 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 42 JFET 302 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. 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). HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Table 42 JFET (Continued) Name Alias Description 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). Table 43 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). HSPICE® Simulation and Analysis User Guide X-2005.09 303 7: Simulation Output Element Template Listings Table 43 MOSFET (Continued) Name Alias Description 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). 304 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. BETAEFF LV21 BETA, effective. GAMMAEFF LV22 GAMMA, effective. DELTAL LV23 ∆L (MOS6 amount of channel length modulation), (valid only for LEVELs 1, 2, 3 and 6). HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Table 43 MOSFET (Continued) Name Alias Description 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). 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 HSPICE® Simulation and Analysis User Guide X-2005.09 305 7: Simulation Output Element Template Listings Table 43 MOSFET (Continued) 306 Name Alias Description 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). – 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). HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Table 43 MOSFET (Continued) Name Alias Description CDGBO LX32 CDGBO = ∂Qd/ ∂Vgb CDDBO LX33 CDDBO = ∂Qd/ ∂Vdb CDSBO LX34 CDSBO = ∂Qd/ ∂Vsb Table 44 Saturable Core 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 45 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 RF supports the output formats in this section: ■ Analog Compression ■ Tabulated Data Output ■ WDB Output Format ■ XP Output Format ■ NW Output Format HSPICE® Simulation and Analysis User Guide X-2005.09 307 7: Simulation Output Element Template Listings ■ VCD Output Format ■ Turbowave Output Format ■ Undertow Output Format ■ .GEN Output Format If your netlist includes an unsupported output format, HSPICE RF prints a warning message, indicating that the selected format is not supported. HSPICE RF then defaults the output to WDB format. You can use the waveform viewer to view certain output formats: ■ WDB#: XP/Cosmos Scope (Recommended) ■ NW#: XP/Avanwaves ■ XP#: XP/Avanwaves/Cosmos Scope Note: If the waveform file is larger than 2GB, use split waveforms. Analog Compression Analog compression eliminates unnecessary data points from a HSPICE RF voltage or current waveform, to reduce the size of the waveform file. SIM_DELTAV (Voltage) To determine the selection criteria for HSPICE RF voltage waveforms in the WDB or NW format, set a SIM_DELTAV value. During simulation, HSPICE RF checks whether the value of the X signal at the n timestep changes by more than the SIM_DELTAV option, from its previous value at the n-1 timestep. ■ If yes, then HSPICE RF saves the new data point. ■ Otherwise, this new data point is lost. Typically such an algorithm yields a reduced file size, with minimal resolution loss, as long as you set an appropriate SIM_DELTAV value. If a value for the SIM_DELTAV option is too large, the waveform degrades. 308 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Element Template Listings Figure 44 Analog Compression Formats NW retains these data points that are ON the line, plotting 3 segments. But NW and WDB both eliminate these data points, WDB eliminates these data which are within DELTAV or DELTAI of the previous points, plotting only ONE data point, and are not ON the plotted waveform line. segment for this line. Example In the following example, at the n timestep, HSPICE RF saves only datapoints that change by more than 1 millivolt (the default), from their previous values at the n-1 timestep. .OPTION SIM_DELTAV = 1mv SIM_DELTAI (Current) You can also specify selective storage on HSPICE RF current waveforms in the WDB or NW format, using SIM_DELTAI. In the following example, at the n timestep, HSPICE RF saves only datapoints that change by more than 0 amps (the default), from their previous values at the n-1 timestep. .OPTION SIM_DELTAI = 0amps Tabulated Data Output HSPICE RF outputs all analog waveforms that you specified in the .PRINT statements. HSPICE RF saves these waveforms as ASCII tabulated data, into a file with the .PRINT extension. To display waveforms graphically, Cosmos-Scope can directly read the tabulated data. For more information about Cosmos-Scope, see the CosmosScope User’s and Reference Manual. Note: Tabulated data excludes waveforms specified in .PROBE statements. HSPICE® Simulation and Analysis User Guide X-2005.09 309 7: Simulation Output Element Template Listings WDB Output Format Waveform database (WDB) output is the default format for the POST option. It was developed for maximum efficiency. The output file is *.wdb0. Signals across multiple hierarchies, that map to the same node, are named together. They also share the same waveform data. You can also set-up the database, so that Cosmos-Scope extracts one signal at a time. This means that Cosmos-Scope does not need to read the entire output files, to display a single waveform. Example .OPTION POST = wdba The WDB format was designed to make accessing waveform data faster and more efficient. It is a true database, so the waveform browser does not have to load the complete waveform file for you to view a single signal. This feature is especially useful if the size of the waveform file is several gigabytes. Furthermore, the WDB format is more compact than XP and NW, which are described later in this section. However, if the NW file is already very small, then WDB offers little advantage in size or speed. XP Output Format HSPICE RF outputs the XP binary format to a file with the .xp# extension. This format is compatible with the HSPICE tr# binary format. The syntax to output a *.xp# file in XP format is: .OPTION POST = xp NW Output Format HSPICE RF outputs the NW format to a file with the extension .nw#. This format was developed by Synopsys, so you need the AvanWaves waveform display tool to process a file in NW format. The syntax to output a *.nw# file in NW format is: .OPTION POST = nw 310 HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Limiting Output Data Size in HSPICE RF VCD Output Format To output your waveforms in VCD (Value Change Dump) format, set the VCD option, in conjunction with the .LPRINT statement. .OPTION VCD .LPRINT (0.5 4.5) v(0) v(2) v(6) Turbowave Output Format To use Turbowave output format: .OPTION POST=tw This format supports analog compression, as described in Analog Compression on page 308. Undertow Output Format To use Veritools Undertow output format: .OPTION POST=ut Limiting Output Data Size in HSPICE RF For multi-million transistor simulations, an unrestricted waveform file can grow to several gigabytes in size. The file becomes unreadable in some waveform viewers, and requires excessive space on the hard drive. This section describes options that limit the number of nodes output to the waveform file, to reduced the file size. HSPICE RF supports the following options to control the output: ■ SIM_POSTTOP Option ■ SIM_POSTSKIP Option ■ SIM_POSTAT Option ■ SIM_POSTDOWN Option ■ SIM_POSTSCOPE Option HSPICE® Simulation and Analysis User Guide X-2005.09 311 7: Simulation Output Limiting Output Data Size in HSPICE RF SIM_POSTTOP Option The SIM_POSTTOP option limits the data written to your waveform file, to data from only the top n level nodes. Note: To enable the waveform display interface, you also need the POST option. Example .OPTION SIM_POSTTOP = n ■ Default value = 3 ■ This syntax outputs instances from up to n levels deep. ■ SIM_POSTTOP = 1 specifies to output only the top-level signals. ■ If you specify the PROBE option, without the SIM_POSTTOP option, then HSPICE RF sets the SIM_POSTTOP = 0. ■ If you do not specify either the PROBE or the SIM_POSTTOP option, then HSPICE RF outputs all levels. SIM_POSTSKIP Option This option specifies that SIM_POSTTOP should skip any instances, and their children, that the subckt_definition defines. To specify more than one definition, use this option once for each definition to skip. Syntax .OPTION SIM_POSTSKIP = subckt_definition SIM_POSTAT Option The SIM_POSTAT option limits the waveform output to only the nodes in the specified subcircuit instance. 312 ■ This option has precedence over SIM_POSTSKIP. ■ You can use this option in conjunction with SIM_POSTTOP. ■ To specify multiple instances, you can either use wildcards, or set the option multiple times. HSPICE® Simulation and Analysis User Guide X-2005.09 7: Simulation Output Limiting Output Data Size in HSPICE RF Syntax .OPTION SIM_POSTAT = instance This syntax includes an instance in the output. SIM_POSTDOWN Option This option includes an instance, and all children of that instance, in the output. SIM_POSTDOWN is identical to SIM_POSTAT, except that SIM_POSTDOWN includes all children of the specified level. Syntax .OPTION SIM_POSTDOWN = instance SIM_POSTSCOPE Option Use this option to specify the signals to probe, from within a scope. Syntax .OPTION SIM_POSTSCOPE = net|port|all ■ Default value = net ■ net indicates to output only nets in the scope. ■ port indicates to output both nets and ports. ■ all indicates to output nets, ports, and global variables. Examples Refer to Figure on page 314 when you examine the following examples. ■ This example specifies to output all nets: .OPTION POST ■ This example outputs top, X1, and X2: .OPTION SIM_POSTTOP = 2 ■ This example outputs top, and skips X2. X1, because it is an instance of the ADD sub-circuit: .OPTION SIM_POSTTOP = 2 .OPTION SIM_POSTSKIP = ADD HSPICE® Simulation and Analysis User Guide X-2005.09 313 7: Simulation Output Node Hierarchy ■ This example outputs X1.X4: .OPTION SIM_POSTAT = X1.X4 ■ This example outputs top, X1, X1.X4, X1.X4.X1, X1.X4.X2, and X2: .OPTION SIM_POSTTOP = 2 .OPTION SIM_POSTDOWN = X1.X4 Node Hierarchy top X1(ADD) 314 X5 X4 X3 X1 X2(SUB) X2 X1 X6 X2 HSPICE® Simulation and Analysis User Guide X-2005.09 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 manual. Simulation Flow Figure 45 shows the simulation flow for DC analysis in Synopsys HSPICE and HSPICE RF. HSPICE® Simulation and Analysis User Guide X-2005.09 315 8: Initializing DC/Operating Point Analysis Initialization and Analysis Figure 45 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. 316 HSPICE® Simulation and Analysis User Guide X-2005.09 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. 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. Figure 46 Equivalent Voltage Source: NODESET and .IC I=GMAX*V HSPICE® Simulation and Analysis User Guide X-2005.09 GMAX To Initialization Node 317 8: Initializing DC/Operating Point Analysis Initialization and Analysis 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. When you set initial conditions for Transient Analysis: 318 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis DC Initialization and Operating Point Calculation ■ 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 + 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 HSPICE® Simulation and Analysis User Guide X-2005.09 0:VPCE 0:VP7 319 8: Initializing DC/Operating Point Analysis DC Initialization and Operating Point Calculation VOLTS 0 5.00000 0 -5.00000 AMPS -2.07407U -405.41294P 2.07407U POWER 0. 2.02706N 0. 2.02706N 405.41294P 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. ■ HSPICE RF does not support this option, so IC is always set to IC=OFF. Example This example describes an H element dependent-voltage source: HXCC 13 20 VIN1 VIN2 IC = 0.5, 1.3 320 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis DC Initialization and Operating Point Calculation 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. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 321 8: Initializing DC/Operating Point Analysis DC Initialization and Operating Point Calculation 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 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. 322 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis .DC Statement—DC Sweeps .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 X-2005.09 323 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: 324 ■ Absolute and relative voltages. ■ Current tolerances. ■ Matrix options. HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Accuracy and Convergence Use .OPTION statements to specify the following options, which control DC analysis: 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 HSPICE® Simulation and Analysis User Guide X-2005.09 325 8: Initializing DC/Operating Point Analysis Accuracy and Convergence convergence loop. For each iteration of the convergence loop, HSPICE or 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 46 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 328 describes the options in Table 46. Table 46 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. 326 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Accuracy and Convergence Note: ABSMOS and RELMOS are the tolerances for MOSFET drain currents. 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 47 shows an example of the relationship between the RELVDC value, and the number of iterations. Table 47 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 HSPICE® Simulation and Analysis User Guide X-2005.09 327 8: Initializing DC/Operating Point Analysis Accuracy and Convergence 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 354. ABSH DCON RELH ABSI DCTRAN RELI ABSMOS DI RELMOS 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 47 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. 328 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Accuracy and Convergence Figure 47 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 Results 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 Results N 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. Try CONVERGE=1 Converged? Y Results N 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. Try CONVERGE=4 Y Converged? Results N Non-convergence report Referring to Figure 47: ■ Setting .OPTION DCON = -1 disables steps 2 and 3. ■ Setting .OPTION CONVERGE = -1 disables steps 4 and 5. HSPICE® Simulation and Analysis User Guide X-2005.09 329 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 47. GMINDC for various elements is shown in Figure 48. 330 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Accuracy and Convergence Figure 48 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 X-2005.09 331 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. 332 • 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 X-2005.09 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 X-2005.09 333 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 49 on page 335, HSPICE or HSPICE RF inserts conductance (G), in parallel with capacitance (Cg). This provides current paths around capacitances, in DC analysis. 334 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Diagnosing Convergence Problems Figure 49 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 X-2005.09 335 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, which lists all non-convergent elements, and their associated element currents, element voltages, model parameters, and current error tolerances (tol). 1. To locate the branch current or nodal voltage that causes non-convergence, 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 sub-circuit, model, and element name for all parts of the circuit where node voltages or currents do not converge. For example, Table 48 identifies the xinv21, xinv22, xinv23, and xinv24 inverters, as problem sub-circuits in a ring oscillator. It also indicates that the pchannel 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 48, 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 336 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Diagnosing Convergence Problems vbs). Examine whether these values are realistic, and determine the transistor regions of operation. Table 48 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 653.8030 m 745.5860 m 732.8632 m 549.4114 m 656.5097 m tolds 114.8609 82.5624 155.9508 104.5004 5.3653 tolbd 0. 0. 0. 0. 0. tolbs 3.534e-19 107.1528 m 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 HSPICE® Simulation and Analysis User Guide X-2005.09 337 8: Initializing DC/Operating Point Analysis Diagnosing Convergence Problems 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 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 statement), 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 50 Ring Oscillator .IC V(1)=5V 1 338 2 3 4 5 HSPICE® Simulation and Analysis User Guide X-2005.09 8: Initializing DC/Operating Point Analysis Diagnosing Convergence Problems The best way to set up the flip-flop is to use an .IC statement in the subcircuit definition. 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 X-2005.09 339 8: Initializing DC/Operating Point Analysis Diagnosing Convergence Problems Figure 51 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. 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. 340 HSPICE® Simulation and Analysis User Guide X-2005.09 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 X-2005.09 341 8: Initializing DC/Operating Point Analysis Diagnosing Convergence Problems 342 HSPICE® Simulation and Analysis User Guide X-2005.09 9 Transient Analysis 9 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 52 illustrates the simulation flow for transient analysis in Synopsys HSPICE and HSPICE RF. HSPICE® Simulation and Analysis User Guide X-2005.09 343 9: Transient Analysis Overview of Transient Analysis Figure 52 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: 344 ■ 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 X-2005.09 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. Syntax .OPTION SIM_ACCURACY = value Default value = 1. In this syntax, value is a positive number. If you specify .OPTION ACCURATE, then the default value is 10. This option is applicable for all modes. SIM_ACCURACY tightens all tolerances, such as: ■ Newton-Raphson tolerance. ■ Local truncation error. ■ Other errors. The default is calibrated to provide good out-of-the-box accuracy, with good performance. HSPICE RF supports this syntax; HSPICE does not. HSPICE® Simulation and Analysis User Guide X-2005.09 345 9: Transient Analysis Overview of Transient Analysis You can apply different accuracy settings to different blocks or time intervals. To set global accuracy, use: .OPTION SIM_ACCURACY = n In this syntax, n is a number greater than 0. The syntax to set accuracy on a block, instance, or time interval is similar to SIM_V_SUPPLY. Example This example sets accuracy to 3 for the XNAND1 and XNAND2 instances, and accuracy to 4 for all instances of the INV subcircuit. Globally, the accuracy is 2. If accuracy settings conflict, then HSPICE RF uses the higher accuracy value. At 12.0ns before the end of the simulation, the global accuracy level is 5. Because this is higher than 2, 3, or 4, it overrides all previous settings. .OPTION SIM_ACCURACY = 2 .OPTION SIM_ACCURACY = “3 | XNAND1 XNAND2” .OPTION SIM_ACCURACY = “4 | @INV” .OPTION SIM_ACCURACY = “5 | 12.0n” Note: SIM_ACCURACY has precedence over ACCURATE. 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 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. 346 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Transient Analysis of an RC Network Parameter *.print Description Writes the output from the .PRINT statement to a *.print file. HSPICE does not generate a *.print# file. • 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. *.tr# Writes output from the .PROBE, .PRINT, .PLOT, .GRAPH, or .MEASURE statement to a *.tr# file. Transient Analysis of an RC Network You can run a transient analysis, using an 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 You can find the complete netlist for this example in the following directory: $installdir/demo/hspice/apps/quickTRAN.sp Note: The V1 source specification includes a pulse source. For the syntax of pulse sources and other types of sources, seeChapter 5, “Sources and Stimuli.”. 1. To run HSPICE, type the following: hspice quickTRAN.sp > quickTRAN.lis HSPICE® Simulation and Analysis User Guide X-2005.09 347 9: Transient Analysis Transient Analysis of an Inverter 2. To examine the simulation results and status, use an editor and view the .lis and .st0 files. 3. Run AvanWaves and open the .sp file. 4. To view the waveform, select the quickTRAN.tr0 file from the Results Browser window. 5. Display the voltage at nodes 1 and 2 on the x-axis. Figure 53 on page 348 shows the waveforms. Figure 53 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) 1.40u 1.60u 1.80u 2.0u Transient Analysis of an Inverter As a final example, analyze the behavior of the simple MOS inverter shown in Figure 54. 348 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Transient Analysis of an Inverter Figure 54 MOS Inverter Circuit VCC VCC + _ M1 IN VIN OUT CLOAD 0.75 pF + _ M2 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 the following 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. Figure 55 shows the waveforms. HSPICE® Simulation and Analysis User Guide X-2005.09 349 9: Transient Analysis Using the .BIASCHK Statement Figure 55 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 0.0 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 analysis, and reports: ■ Element name ■ Time ■ Terminals ■ Bias that exceeds the limit ■ Number of times the bias exceeds the limit for an element 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 the .BIASCHK statement. The following limitations apply to the .BIASCHK command: 350 ■ .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. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Using the .BIASCHK Statement ■ Wildcards in element and model names, and except definitions are supported but not in expressions. See the HSPICE Command Reference for more information about the .BIASCHK command. 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) 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. HSPICE® Simulation and Analysis User Guide X-2005.09 351 9: Transient Analysis Using the .BIASCHK Statement 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. 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. 352 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Transient Control Options Example The following example is a netlist that uses the .BIASCHK command for a transient simulation. You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/apps/biaschk.sp 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). Table 49 Transient Control Options, Arranged by Category Method Tolerance BYPASS CSHUNT DVDT GSHUNT INTERP ITRPRT LVLTIM MAXORD METHOD POST* PROBE* PURETPSIM_ ORDER* RUNLVL SIM_TRAP* TRCON ABSH ABSV ABSVAR ACCURAT E BYTOL CHGTOL DI FAST MBYPASS MAXAMP MU RELH RELI RELQ RELTOL RELV Limit RELVAR SIM_ACCURACY* SIM_DELTAI* SIM_DELTAV* SIM_MAXSTEP* 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 HSPICE® Simulation and Analysis User Guide X-2005.09 353 9: Transient Analysis Simulation Speed and Accuracy 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. 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. 354 ■ .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. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Simulation Speed and Accuracy 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 = 4LVLTIM = 1RMAX = 5SLOPETOL = 0.75 FT = FS = 0.25BYPASS = 1BYTOL = MBYPASSxVNTOL = 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. 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 366. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 355 9: Transient Analysis Simulation Speed and Accuracy 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 50. DVDT = 2 BYTOL = 0 RELVAR = 0.2 LVLTIM = 3 BYPASS = 0 ABSVAR = 0.2 FT = FS = 0.2 RMAX = 2 RELMOS = 0.01 SLOPETOL = 0.5 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, NRS, to override the default calculations. ■ 356 CAPOP = 4 models the most advanced charge conservation, nonreciprocal 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. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Linear Acceleration (SIM_LA Option) 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). 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. Linear Acceleration (SIM_LA Option) HSPICE RF provides a linear acceleration capability, using the SIM_LA option. HSPICE does not support this option. SIM_LA accelerates simulation of circuits that include large linear RC networks. To do this, HSPICE RF 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. Both the main circuit elements (including .PRINT, .PROBE, and .MEASURE elements), and the RC elements, share 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, a relationship represented by the multiport admittance of a network. HSPICE® Simulation and Analysis User Guide X-2005.09 357 9: Transient Analysis Linear Acceleration (SIM_LA Option) 1. The SIM_LA option formulates matrices, to represent multiport admittance. 2. 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. Multiport Admittance vs. Frequency admittance Figure 56 ce tan t i dm al a u t ac approx f0 frequency 3. The amount of reduction depends on the specified upper frequency f0, which is the threshold frequency where SIM_LA preserves the admittance. For frequencies below f0, the approx signal matches 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. You can choose one of two algorithms, explained below: ■ 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. 358 ■ The transform preserves the first two moments of admittance at DC (slope and offset), so that DC behavior is correct (see Figure 57 on page 359). ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Linear Acceleration (SIM_LA Option) This approach is the most accurate of the two algorithms, and is the default. PACT Algorithm ed erv s pre et s f of nd ce a tan e t i p slo adm ual t c a admittance Figure 57 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. Syntax The syntax for choosing between the two algorithms is: .OPTION SIM_LA = PACT | PI Default value = PACT If you set the entire netlist to ANALOG mode, the linear matrix is not reduced. HSPICE® Simulation and Analysis User Guide X-2005.09 359 9: Transient Analysis Linear Acceleration (SIM_LA Option) Specifying Maximum Resistance You can control the maximum resistance to preserve. Syntax .OPTION SIM_LA_MAXR = value Default value = 1e15 ohms In this syntax, 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. Specifying Minimum Capacitance You can specify the minimum capacitance to preserve. Syntax .OPTION SIM_LA_MINC = value Default value = 1e-16 farads. In this syntax, value is the minimum capacitance preserved in the reduction. After reduction completes, SIM_LA lumps any capacitor smaller than value, to ground. Other PACT Options (HSPICE RF) HSPICE RF provides four additional PACT options. Specifying Error Tolerance You can specify the error tolerance. Syntax .OPTION SIM_LA_TOL = value Default value = 0.05 In this syntax, value (the error tolerance for the PACT algorithm) is a value between 0.0 and 1.0. 360 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Linear Acceleration (SIM_LA Option) Specifying Upper Frequency You can specify the upper frequency. Syntax .OPTION SIM_LA_FREQ = value Default value = 1 GHz In this syntax, value is the upper frequency for which the PACT algorithm must preserve accuracy. If value is 0, then 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. Specifying Minimum Switching Time As an alternative to SIM_LA_FREQ, you can specify the minimum switching time. Syntax .OPTION SIM_LA_TIME = value Default value = 1ns In this syntax, value is the minimum switching time for which the PACT algorithm preserves accuracy. Waveforms that occur more rapidly than this time, are not accurately represented. SIM_LA_TIME is simply the dual of SIM_LA_FREQ. The default is equivalent to setting SIM_LA_FREQ = 1 GHz. Example 1 A circuit has a typical rise time of 1ns, so set the maximum frequency to 1 GHz, or set the minimum switching time to 1ns: .OPTION SIM_LA_FREQ = 1 GHz or .OPTION SIM_LA_TIME = 1ns HSPICE® Simulation and Analysis User Guide X-2005.09 361 9: Transient Analysis Linear Acceleration (SIM_LA Option) However, if spikes occur in 0.1ns, HSPICE RF does not accurately simulate them. To capture the behavior of the spikes, use: .OPTION SIM_LA_FREQ = 10 GHz or .OPTION SIM_LA_TIME = 0.1ns Note: Higher frequencies (smaller times) increase accuracy, but only up to the minimum time step used in HSPICE RF. Node Reduction To reduce the number of nodes, instead of the number of elements, use the SIM_LA_MINMODE option. Syntax .OPTION SIM_LA_MINMODE = ON|OFF SIM_LA Options Summary 362 Parameter Description SIM_LA Activates linear matrix reduction, and selects between four methods. Default is PACT. SIM_LA_FREQ Upper frequency for which accuracy must be preserved. Default=1 GHz. SIM_LA_MAXR Maximum resistance for linear matrix reduction. Default is 1e15 ohms. SIM_LA_MINC Minimum capacitance for linear matrix reduction. Default=1e16 farads. SIM_LA_TIME Minimum time for which accuracy must be preserved. This is a dual of SIM_LA_FREQ. Default is 1ns. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Numerical Integration Algorithm Controls (HSPICE) Parameter Description SIM_LA_TOL Error tolerance for the PACT algorithm. Default is 0.05. SIM_LA_MINMODE Reduces the number of nodes, instead of the number of elements. Numerical Integration Algorithm Controls (HSPICE) 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. HSPICE® Simulation and Analysis User Guide X-2005.09 363 9: Transient Analysis Numerical Integration Algorithm Controls (HSPICE) Figure 58 Time Domain Algorithm Initialization.IC NODESET Iteration Solution Converged Reversal Time Step Algorithm Advancement (tnew = told + ∆t) 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. 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). 364 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Numerical Integration Algorithm Controls (HSPICE) ■ Set .OPTON METHOD=TRAP in the netlist, then manually adjust TSTEP and the relevant control options (such as CSHUNT or GSHUNT). Figure 59 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 HSPICE® Simulation and Analysis User Guide X-2005.09 365 9: Transient Analysis Numerical Integration Algorithm Controls (HSPICE RF) Numerical Integration Algorithm Controls (HSPICE RF) In HSPICE RF, you can select either the Backward-Euler or Trapezoidal integration algorithm. Each of these algorithms has its own advantages and disadvantages for specific circuit types. For pre-charging simulation or timing critical simulation, the Trapezoidal algorithm usually improves accuracy. x Default value = 1.9 In this syntax, x is a real number between 1.0 and 2.0. Note: SIM_ORDER has precedence over SIM_TRAP. ■ A higher order is more accurate, especially with inductors (such as crystal oscillators), which need SIM_ORDER = 2.0. ■ A lower order has more damping. Setting SIM_ORDER to its lowest value, as in the example below, selects the Backward-Euler integration algorithm. .OPTION SIM_ORDER = 1.0 Selecting Timestep Control Algorithms In HSPICE or HSPICE RF, you can select one of three dynamic timestepcontrol algorithms: ■ Iteration Count Dynamic Timestep Algorithm ■ Local Truncation Error (LTE) Dynamic Timestep ■ DVDT Dynamic Timestep Algorithm 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. 366 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Selecting Timestep Control Algorithms Figure 60 Internal Variable Timestep Changing Time Step - Dynamic ∆tD-1 ∆tD 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 Algorithm on page 368. ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 367 9: Transient Analysis Selecting Timestep Control Algorithms Iteration Count Dynamic Timestep Algorithm The simplest dynamic timestep algorithm is the iteration count algorithm. .OPTION IMAX and .OPTION IMIN control this algorithm. Local Truncation Error (LTE) Dynamic Timestep The local truncation error timestep method uses a Taylor-series approximation, to calculate the next timestep for a transient analysis. This method uses the allowed local truncation error, to calculate an internal timestep. 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. To select the timestep algorithm for local truncation error, 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 Algorithm To select this algorithm, set the LVLTIM option to 1 or 3. ■ 368 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. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Selecting Timestep Control Algorithms ■ 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 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 with HSPICE Release 95.3, use these options. Setting .OPTION DVDT = 3 automatically sets all of these values. HSPICE® Simulation and Analysis User Guide X-2005.09 369 9: Transient Analysis Selecting Timestep Control Algorithms 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 algorithm. If the timestep is below the minimum, program execution stops. Example If the timestep becomes less than the minimum internal timestep (defined as TSTEP x RMIN), HSPICE reports an internal timestep too small error. Note: RMIN is the minimum timestep coefficient. Default is 1e-9. TSTEP is the time increment set in the .TRAN statement. 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, (TSTEPxRMAX)] 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), HSPICE might activate autospeedup. This process automatically sets RMAX to a bigger value, and sets the maximum internal timestep to: min[(TSTOP/20),(TSTEPxRMAX)] 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 correspondinglylarge 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 370 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Selecting Timestep Control Algorithms control, so setting a high SLOPETOL reduces the number of usable breakpoint table entries, which reduces the simulation time. Timestep Control in HSPICE RF This section describes Timestep Control options in HSPICE RF. ■ The default time step method mixes Trapezoidal and Gear-2. This yields a more accurate scheme than Trapezoidal and BE. ■ Detection of numerical oscillations inserts fewer BE steps than in previous HSPICE versions. .OPTION SIM_ACCURACY To modify the size of timesteps in HSPICE RF, use the SIM_ACCURACY option. A timestep is a time interval at which you evaluate a signal. HSPICE RF discretely expresses the time continuum as a series of points. At each point or timestep, a circuit simulator evaluates the corresponding voltage or current value of a signal. Thus, a resulting signal waveform is a series of individual data points; connecting these points results in a smooth curve. Syntax .OPTION SIM_ACCURACY = value Default value = 1 where value is a positive number. If you specify .OPTION ACCURATE, then the default value is 10. This option applies to all modes. SIM_ACCURACY tightens all tolerances, such as: ■ Newton-Raphson tolerance. ■ Local truncation error. ■ Other errors. The default is calibrated to provide good out-of-the-box accuracy, with good performance. You can apply different accuracy settings to different blocks or time intervals. To set global accuracy, use: .OPTION SIM_ACCURACY = n In this syntax, n is a number greater than 0. The syntax to set accuracy on a block, instance, or time interval is similar to SIM_V_SUPPLY. HSPICE® Simulation and Analysis User Guide X-2005.09 371 9: Transient Analysis Selecting Timestep Control Algorithms Example This example sets accuracy to 3 for the XNAND1 and XNAND2 instances, and accuracy to 4 for all instances of the INV subcircuit. Globally, the accuracy is 2. If accuracy settings conflict, then HSPICE RF uses the higher accuracy value. At 12.0ns before the end of the simulation, the global accuracy level is 5. Because this is higher than 2, 3, or 4, it overrides all previous settings. .OPTION SIM_ACCURACY = 2 .OPTION SIM_ACCURACY = .OPTION SIM_ACCURACY = .OPTION SIM_ACCURACY = .OPTION SIM_ACCURACY = .OPTION SIM_ACCURACY = .OPTION SIM_ACCURACY = “3 “4 “5 “5 “3 “5 | | | | | | XNAND1 XNAND2” @INV” 12.0n” 20n” 40ns” 20ns 3 | 35ns 7 | 50ns” Default value = infinity. Note: SIM_ACCURACY has precedence over ACCURATE. .OPTION METHOD To select a timestep control option, select the METHOD option. HSPICE RF supports three basic time step algorithms: Trapezoidal, secondorder Gear (Gear-2), and Backward Euler (BE). BE is the same as first-order Gear. HSPICE RF also supports a hybrid algorithm, which is a mixture of the three basic algorithms. HSPICE RF contains an algorithm for auto-detection of numerical oscillations commonly encountered with trapezoidal integration. If HSPICE RF detects such oscillations, it inserts BE steps, but not more than one BE step for every 10 time steps. To turn off auto-detection, use the PURETP option. Syntax .OPTION METHOD = [TRAP | GEAR | TRAPGEAR] 372 ■ TRAP selects the trapezoidal algorithm. ■ GEAR selects the Gear algorithm. ■ TRAPGEAR (default) selects a hybrid method. HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Selecting Timestep Control Algorithms .OPTION MAXORD Selects the maximum order of integration for the GEAR method. ■ 1=first-order Gear (Backward Euler). ■ 2=second-order Gear (Gear-2) .OPTION SIM_ORDER Controls the amount of BE to mix with the Trapezoidal method for hybrid integration. It affects time stepping when you set method to trap or trapgear. ■ SIM_ORDER=1 is BE. ■ SIM_ORDER=2 (default) is Trapezoidal. ■ Any real number from 1 to 2 is valid. .OPTION SIM_TG_THETA For the hybrid TRAPGEAR method, controls the amount of Gear-2 method to mix with trapezoidal integration. Default=0.1. ■ SIM_TG_THETA=0 selects trapezoidal without Gear-2. ■ SIM_TG_THETA=1 selects pure Gear-2. ■ Any real number from 0 to 1 is valid. .OPTION SIM_TRAP Changes the default SIM_TG_THETA to 0, so that method=trapgear acts like METHOD=TRAP. You can set this flag to 0 (default) or 1. .OPTION PURETP Turns off insertion of BE steps, due to auto-detection of numerical oscillations. You can set this flag to 0 (default) or 1. .OPTION SIM_OSC_DETECT_TOL Tolerance for detecting numerical oscillations. If HSPICE RF detects numerical oscillations, it inserts BE steps. Smaller values of this tolerance result in fewer BE steps. Default=10-8. HSPICE® Simulation and Analysis User Guide X-2005.09 373 9: Transient Analysis Selecting Timestep Control Algorithms Examples The default behavior is a hybrid method, combining 90% trapezoidal with 10% Gear-2. HSPICE RF inserts BE steps, when the simulator encounters a breakpoint, or when the auto-detection algorithm finds numerical oscillations. Example 1 .option method=trap purept This option sets pure trapezoidal method integration. No Gear-2 or BE is mixed in. Use this setting when you simulate harmonic oscillators. Example 2 .option method=gear maxord=1 Sets pure Backward Euler integration. Example 3 .option method=trap sim_order=1 Sets pure Backward Euler integration. Example 4 .option method=gear Sets pure Gear-2 integration. Example 5 .option sim_order=1.9 This causes a mixture of 10% Gear-2 and 90% BE-trapezoidal hybrid integration. The BE-trapezoidal part is 10% BE. 374 HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Fourier Analysis Fourier Analysis This section describes the Fourier and FFT Analysis flow for HSPICE. Figure 61 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. HSPICE® Simulation and Analysis User Guide X-2005.09 375 9: Transient Analysis Fourier Analysis ■ .FFT is a much more flexible Fourier analysis tool. Use it for analysis tasks that require more detail and precision. 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. Example 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 ∑ m=0 C m ⋅ cos ( mt ) + ∑ D m ⋅ sin ( mt ) m=0 The following equations calculate values for the preceding equation: π Cm 1 = --- ⋅ π ∫ g ( t ) Þ cos ( m ⋅ t ) Þdt –π π Dm 376 1 = --- ⋅ π ∫ g ( t ) Þ sin ( m ⋅ t ) Þdt –π HSPICE® Simulation and Analysis User Guide X-2005.09 9: Transient Analysis Fourier Analysis 9 g( t) = 9 ∑ C m ⋅ cos ( m ⋅ t ) + m=0 ∑ D m ⋅ sin ( m ⋅ t ) m=0 The following equations approximate the C and D values: 500 Cm = 2⋅π⋅m⋅n - ∑ g ( n ⋅ ∆ t ) ⋅ cos -------------------------501 n=0 500 Dm = 2⋅π⋅m⋅n - ∑ g ( n ⋅ ∆ t ) ⋅ 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. You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/apps/four.sp 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 no 1 2 3 frequency fourier (hz) component 20.0000x 40.0000x 60.0000x 3.0462 115.7006m 753.0446m 4 80.0000x 77.8910m 5 100.0000x 296.5549m HSPICE® Simulation and Analysis User Guide X-2005.09 normalized phase component (deg) 1.0000 176.5386 37.9817m -106.2672 247.2061m normalized phase (deg) 0. -282.8057 170.7288 -5.8098 25.5697m -125.9511 -302.4897 97.3517m 164.5430 -11.9956 377 9: Transient Analysis Fourier Analysis 6 120.0000x 50.0994m 16.4464m -148.1115 7 140.0000x 125.2127m 41.1043m 157.7399 -18.7987 8 160.0000x 25.6916m 8.4339m 172.9579 -3.5807 9 180.0000x 47.7347m 15.6701m 154.1858 -22.3528 total harmonic distortion = 27.3791 -324.6501 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: 378 ■ output format ■ frequency ■ number of harmonics ■ total harmonic distortion (THD) HSPICE® Simulation and Analysis User Guide X-2005.09 10 AC Sweep and Small Signal Analysis 01 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 See the HSPICE Command Reference for .AC command syntax and examples of all these applications. HSPICE® Simulation and Analysis User Guide X-2005.09 379 10: AC Sweep and Small Signal Analysis AC Small Signal Analysis .AC Control Options You can use the following .AC control options when performing an AC analysis: ■ ABSH ■ ACOUT ■ DI ■ MAXAMP ■ RELH ■ UNWRAP See “Options in HSPICE Netlists” in the HSPICE Command Reference for these AC control options syntax. AC Small Signal Analysis AC small signal analysis in HSPICE or HSPICE RF computes AC output variables as a function of frequency (see Figure 62). 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. 380 HSPICE® Simulation and Analysis User Guide X-2005.09 10: AC Sweep and Small Signal Analysis AC Small Signal Analysis Figure 62 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. HSPICE or HSPICE RF converts capacitor and inductor values to their corresponding admittances: y C = j ω C 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. HSPICE® Simulation and Analysis User Guide X-2005.09 381 10: AC Sweep and Small Signal Analysis AC Analysis of an RC Network 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. AC Analysis of an RC Network Figure 63 shows a simple RC network with a DC and AC source applied. The circuit consists of: 382 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 10: AC Sweep and Small Signal Analysis AC Analysis of an RC Network Figure 63 RC Network Circuit 1 R1 1k V1 10 VDC 1VAC 2 + _ R2 1k C1 0.001 mF 0 The input netlist for the RC network circuit is: 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 You can find the complete netlist for this example in the following directory: $installdir/demo/hspice/apps/quickAC.sp 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 HSPICE® Simulation and Analysis User Guide X-2005.09 383 10: AC Sweep and Small Signal Analysis AC Analysis of an RC Network 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 64 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. Figure 64 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: 384 ■ Input netlist. ■ Details about the elements and topology. HSPICE® Simulation and Analysis User Guide X-2005.09 10: AC Sweep and Small Signal Analysis Other AC Analysis Statements ■ 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 You can use the following commands to perform other types of AC analyses: ■ Using .DISTO for Small-Signal Distortion Analysis ■ Using .NOISE for Small-Signal Noise Analysis ■ Using .SAMPLE for Noise Folding Analysis Use the .NOISE and .AC statements to control the noise analysis of the circuit. 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. See .DISTO in the HSPICE Command Reference for command syntax and examples. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 385 10: AC Sweep and Small Signal Analysis Other AC Analysis Statements 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 Parameter Description onoise Total output noise(HSPICE or HSPICE RF). ink Normal current source due to thermal, shot, or other noise. Zk Equivalent transimpedance between each noise current source and output. N 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 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. 386 HSPICE® Simulation and Analysis User Guide X-2005.09 10: AC Sweep and Small Signal Analysis Other AC Analysis Statements If you specify more than one .NOISE statement in a single simulation, HSPICE or HSPICE RF runs only the last statement. Table 51 .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. See “.SAMPLE” in the HSPICE Command Reference for the command syntax. HSPICE® Simulation and Analysis User Guide X-2005.09 387 10: AC Sweep and Small Signal Analysis Other AC Analysis Statements 388 HSPICE® Simulation and Analysis User Guide X-2005.09 11 Linear Network Parameter Analysis 11 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 manual. .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 HSPICE® Simulation and Analysis User Guide X-2005.09 389 11: Linear Network Parameter Analysis .LIN Analysis 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. The .PRINT/.PROBE/.MEAS output syntax for .LIN supports H (hybrid) parameters and S/Y/Z/H group delay. Figure 65 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). 390 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .LIN 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. <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. • 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_waveform> (Transient analysis) Voltage or power source waveform. Any one of waveforms: AM, EXP, PULSE, PWL, SFFM, or SIN. Multiple transient descriptions are not allowed. HSPICE® Simulation and Analysis User Guide X-2005.09 391 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. • 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. <z0=val> (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. 392 HSPICE® Simulation and Analysis User Guide X-2005.09 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 X-2005.09 393 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 66 shows the block diagram of the mixed mode port element. Figure 66 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.” 394 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .LIN Analysis .LIN Input Syntax For the .LIN command syntax, see the HSPICE Command Reference. .LIN Output Syntax .PRINT | PROBE | AC PARAM(TYPE) ... ■ PARAM can be: Xmn | X(m,n) | LINPARAM ■ X can be: S | Y | Z | H ■ mn refers to a pair of port numbers, where m can be 1 or 2, and n can be 1 or 2. ■ LINPARAM can be: NFMIN,GAMMA_OPT,ZOPT,RN,K_STABILITY_FACTOR,G_MAX, G_MAX_S_OPT,G_MAX_L_OPT,NF,G_AS,VSWR(n),GD ■ TYPE can be: R,I,M,P,PD,PR,DB,DBM ■ In the .PRINT or .PROBE output syntax for .LIN, you can include complex two-port hybrid (H-) parameters: Hmn | Hmn(TYPE) | H(m,n) | H(m,n)(TYPE) m = 1 or 2 n = 1 or 2 TYPE = R, I, M, P, PD, PR, or DB 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 elements. HSPICE® Simulation and Analysis User Guide X-2005.09 395 11: Linear Network Parameter Analysis .LIN Analysis 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. PARAM Definitions 396 ■ S (scattering parameters) ■ Y (admittance parameters) ■ Z (impedance parameters) ■ H (hybrid parameters) ■ NFMIN (noise figure minimum) ■ NF (Noise figure) ■ VN2 (Equivalent input noise voltage squared ■ IN2 (Equivalent input noise current squared) HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .LIN Analysis ■ 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 which 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 which achieves maximum available power gain) ■ G_MAX_GAMMA2 (load reflection coefficient which 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) HSPICE® Simulation and Analysis User Guide X-2005.09 397 11: Linear Network Parameter Analysis .LIN Analysis ■ 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) 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) Multi-Port Scattering (S) Parameters S Parameters represent the ratio of incident and scattered (or forward and reflected) normalized voltage waves. Figure 67 shows a two-port network. Figure 67 Two-Port Network I1 Port=1 398 Z01 I2 + V1 - Two-Port Network + V2 Z02 Port=2 - HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .LIN Analysis 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 .PRINT .PRINT .PRINT AC AC AC AC S11(DB) S21(DB) S12(DB) S22(DB) $ $ $ $ Input return loss Gain Isolation 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 2-port for an arbitrary source impedance. Several output parameter measurements are specific to 2-port networks. .LIN analysis supports 2-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 2-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 2-port quantities. HSPICE® Simulation and Analysis User Guide X-2005.09 399 11: Linear Network Parameter Analysis .LIN Analysis 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 2-port linear network. ■ A series voltage noise source, called Vn, at the input of a noiseless 2-port linear network. ■ A source with impedance, called Zs, that drives this 2-port network. ■ The 2-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). 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. 400 ■ ZCOR: Noise correlation impedance (Complex, Ohms) ■ YCOR: Noise correlation admittance (Complex, Siemens) HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .LIN Analysis 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. ■ 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) 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) HSPICE® Simulation and Analysis User Guide X-2005.09 401 11: Linear Network Parameter Analysis .LIN Analysis 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/.PROBE 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...} In this syntax: 402 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .LIN Analysis 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. HSPICE can output the result of .LIN noise analysis to a .sc*, TOUCHSTONE, or CITIfile. Figure 68 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 noise analysis also makes the following measurements available: Vn 2 R n = ---------4kT In 2 G n = --------4kT 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 HSPICE® Simulation and Analysis User Guide X-2005.09 Z opt = R 2 ------n – ( R cor ) – jX cor Gn Z opt – Z 0 γ I opt = --------------------Z opt + Z 0 403 11: Linear Network Parameter Analysis .LIN Analysis 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). 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. 404 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis RF Measurements From .LIN Group delay is a function of frequency: d ( phase ) gd ( w ) = –-------------------------d(w) In the preceding equation: ■ gd = Group delay at the f frequency, 2 π f = 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 d|r ij | 1- dr ij ------df ----------- = - ----------+ j ------r ij dw |r ij | dw dw 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 ij df- = – 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. HSPICE® Simulation and Analysis User Guide X-2005.09 405 11: Linear Network Parameter Analysis RF Measurements From .LIN 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, unitless) 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) Matching for Optimal Gain 406 ■ 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) HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis RF Measurements From .LIN Noise Measurements ■ 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) 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 HSPICE® Simulation and Analysis User Guide X-2005.09 407 11: Linear Network Parameter Analysis RF Measurements From .LIN 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. 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: 408 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis RF Measurements From .LIN 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 + ∆ K = -------------------------------------------------------2 s 12 s 21 ∆ determines the two-port S matrix calculated from this equation: ∆ = s 11 s 22 – s 12 s 21 An amplifier where K>1 is unconditionally stable at the selected frequency. 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 – ∆ S 11 ∆ = 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): HSPICE® Simulation and Analysis User Guide X-2005.09 409 11: Linear Network Parameter Analysis RF Measurements From .LIN 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 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 ) 410 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis RF Measurements From .LIN 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 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 --------Γ1 = ------------- – --------------- – 1 2 C1 2 C1 2C 1 2 2 B 1 = 1 – s 22 + s 11 – ∆ ∗ C 1 = s 11 – ∆ s22 2 ∆ = 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: HSPICE® Simulation and Analysis User Guide X-2005.09 411 11: Linear Network Parameter Analysis RF Measurements From .LIN 2 2 B 2 = 1 – s 11 + s 22 – ∆ 2 ∗ C 2 = s 22 – ∆ s11 ∆ = 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 ■ 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: 412 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis RF Measurements From .LIN 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, ∆f = 1Hz ). 2 |v n | RN = R n = ----------------4kT 0 ∆ f 2 |i n | GN = G n = ----------------4kT 0 ∆ f 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 |v n | i*n v n ZCOR = ρ n --------- = ------------ = R cor + jX cor 2 2 |i n | |i n | 2 YCOR = ρ n |i n | i nv n * --------- = ------------ = G cor + jB cor 2 2 |v n | |v n | 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 HSPICE® Simulation and Analysis User Guide X-2005.09 1 = Y opt = --------Z opt Gn 2 ------ – B cor – jB cor Rn 413 11: Linear Network Parameter Analysis RF Measurements From .LIN 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 ∆ f ■ 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). ■ 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 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 | 414 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis Extracting Mixed-Mode Scattering (S) Parameters 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 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 keyword in the .PRINT/.PROBE statements specifies the elements in the mixed mode S-parameter matrices: S|Y|Z<xy>nm<(t)> Parameter 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 HSPICE® Simulation and Analysis User Guide X-2005.09 415 11: Linear Network Parameter Analysis Extracting Mixed-Mode Scattering (S) Parameters Parameter Description 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 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, 416 ■ Available: ds,cs ■ Default: ds HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis Extracting Mixed-Mode Scattering (S) Parameters Example 4 p1=single p2=balanced Where, ■ Available: sd,sc ■ Default: sd 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 S12 S13 S14 = = = = SDD11 SDD12 SDC11 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. HSPICE® Simulation and Analysis User Guide X-2005.09 417 11: Linear Network Parameter Analysis Extracting Mixed-Mode Scattering (S) Parameters Output Format and Description Parameter 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 + 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) 0.10000E+09 0. 1.0000 0. 1.0281 ... GammaOpt(P) RN/Zo The 2-port noise section starts with “*” so that you can include this file in your HSPICE or HSPICE RF input netlists. 418 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis Extracting Mixed-Mode Scattering (S) Parameters 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. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 419 11: Linear Network Parameter Analysis .NET Parameter Analysis 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 2-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 .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 420 V I [V1 [I1 the = [Z] [I] = [Y] [V] T = [H] [I1 V2]T I2] T V2] = [S] [V1 I2]T transpose of the M matrix). HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .NET Parameter Analysis 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 69 shows the importance of variables in the .NET statement. Here, Isrc and Vce are the DC biases, applied to the BJT. Figure 69 Parameters with .NET V(2) Isrc I2 1 I1 + - Isrc + + V1 V2 - - Vce This .NET statement provides an incorrect result for the Z parameter calculation: .NET V(2) Isrc When HSPICE or HSPICE RF runs AC analysis, it shorts all DC voltage sources; all DC current sources are open-circuited. As a result, V(2) shorts to ground and its value is zero in AC analysis. This affects the results of the network analysis. In this example, HSPICE or HSPICE RF attempts to calculate the Z parameters (Z11 and Z21), defined as Z11 = V1/I1 and Z21 = V2/I1 with I2=0. The above HSPICE® Simulation and Analysis User Guide X-2005.09 421 11: Linear Network Parameter Analysis .NET Parameter Analysis example does not satisfy the requirement that I2 must be zero. Instead, V2 is zero, which results in incorrect values for Z11 and Z21. Figure 70 shows the correct biasing configurations for performing network analysis for the Z, Y, H, and S parameters. Figure 70 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 + V1 - + V1 - + V2 - VCE S-parameter: .NET V(C) VBE I2 C I1 IB 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 422 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .NET Parameter Analysis 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. 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 You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/bjt/net_ana.sp Other possible biasing configurations for the network analysis are: $S-parameter .NET v(c) vbb rin = 50 rout = 50 ve e 0 0 vbb b 0 dc = 'vbe' ac = 0.1 icc 0 c 'ic' q1 c b e 0 bjt $Z-parameter .NET v(c) ibb rin = 50 rout = 50 ve e 0 0 ibb 0 b dc = 'ib' ac = 0.1 icc 0 c 'ic' q1 c b e 0 bjt $Y-parameter .NET i(vc) vbb rin = 50 rout = 50 ve e 0 0 vbb b 0 'vbe' ac = 0.1 vc c 0 'vce' q1 c b e 0 bjt HSPICE® Simulation and Analysis User Guide X-2005.09 423 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) 424 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis .NET Parameter Analysis Bandpass Netlist: Network Analysis Results You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/filters/fbpnet.sp Figure 71 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 -40.0 179.141 100.0 FBPL.AC0 S11[PHASE] 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 X-2005.09 425 11: Linear Network Parameter Analysis References Figure 72 ZIN Magnitude and Phase Plots BAND-PASS NETLIST: HSPICE NETWORK ANALYSIS RESULTS 04/14/2003 18:31:54 120.0 FBPL.AC0 ZIN[MAG 100.0 80.0 60.0 ZIN [LIN] 40.0 FBPL.AC0 ZIN[PHASE 20.0 90_0 50_0 0 -50_0 -90_0 200.0x 220.0x 240.0x 260.0x 280.0x 300.0x HERTZ [LIN] 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. 426 HSPICE® Simulation and Analysis User Guide X-2005.09 11: Linear Network Parameter Analysis References 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.geocities.com/ billbeale0179/Accelerant/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 X-2005.09 427 11: Linear Network Parameter Analysis References 428 HSPICE® Simulation and Analysis User Guide X-2005.09 12 Using HSPICE with Verilog-A 21 Describes how to use Verilog-A in HSPICE simulations. 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 to VerilogAMS LRM2.1 from Accellera with some LRM2.2 features added, such as $table_model, $param_given, output parameters, and the above function. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 429 12: Using HSPICE with Verilog-A Getting Started Getting Started This section explains how to get started using a compact device model written in Verilog-A in HSPICE. Verilog-A devices use the following conventions: ■ modules are loaded into the simulator with either the .hdl netlist command or the –hdl HSPICE command-line option. ■ modules are instantiated in the same manner as HSPICE sub-circuits. 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 (for example, C, D, NMOS, PMOS, and so on). 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. Note: Before you run a circuit with a Verilog-A module, check to be sure that your environment has been set up to source the cshrc.meta file. For details, see the HSPICE chapter to the Installation Guide. 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 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; 430 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Getting Started 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 sub-circuit 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. The parameter passed in from the netlist is tested during the simulation and a run- time error occurs if the parameter is out of the allowed range. The device is used in the HSPICE netlist in exactly the same manner that a built-in device is used. The netlist example shown in below performs a simple DC-IV analysis. Verilog-A version of the SPICE JFET .hdl jfet.va .options post=1 VCC Drain 0 3.0 HSPICE® Simulation and Analysis User Guide X-2005.09 431 12: Using HSPICE with Verilog-A Getting Started VG VS Gate 0 Source 0 0.5 0.0 X1 Drain Gate Source jfet Vto=-2.0 Beta=1.1e-4 Lambda=0.01 .dc VCC 0.0 4.0 0.01 VG -2.0 0.0 0.5 .print I(VCC) .end When the simulation is performed, the program compiles the Verilog-A source file into a compiled object file. This object file is automatically cached and subsequent simulations do not require the compile step unless the Verilog-A source file is modified. After simulation, HSPICE outputs the data in the same fashion as other devices. In this example the drain-source current is plotted as a function of Vds and parameterized by Vgs. Figure 73 displays the plot of the drain-source current for this model. Figure 73 432 IV Characteristics of a Verilog-A JFET HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Introduction to Verilog-A Introduction to Verilog-A The following is a Verilog-A module example provides an overview of the language. See the Verilog-AMS LRM2.1 from Accellera for syntax and usage details. Verilog-A Module Template The following basic template illustrates basic of the language's features. `include "disciplines.vams" // Natures and disciplines `include "constants.vams" // Common physical and math // constants module my_model(port1, bus); electrical port1; electrical [0:1] bus; parameter real real_param = 1.0 from [0:inf); parameter integer int_param = 1 from [-1:1] exclude 0; real real_var; analog begin @ ( 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 HSPICE® Simulation and Analysis User Guide X-2005.09 433 12: Using HSPICE with Verilog-A Introduction to Verilog-A Data Types Four Verilog-A data types are available. The parameter type is used to pass values from the netlist to the module. Table 52 Verilog-A Data Types Data Type Description integer Discrete numerical type integer integer_name {, integer_name}; genvar Special integer-valued variable for behavioral looping constructs genvar genvar_name {, genvar_name}; real Continuous numerical type real real_name {, real_name}; 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 ] ] ; Analog Operators and Filters Analog operators and filters maintain memory states of past behavior. They can not be used in an analog function. Table 53 Verilog-A Analog Operators and Filters Operator Function 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 ] ] ] ) 434 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Introduction to Verilog-A Table 53 Verilog-A Analog Operators and Filters (Continued) Operator Function 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 zeropole form of the Laplace transform filter. laplace_*(expr, u, v) HSPICE® Simulation and Analysis User Guide X-2005.09 435 12: Using HSPICE with Verilog-A Introduction to Verilog-A Table 53 Verilog-A Analog Operators and Filters (Continued) Operator Function Z-transform filters The Z-transform filters implement linear discrete-time filters. All Z-transform 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 Z-transform filter. • zi_zp() implements the zero-pole form of the Z-transform filter. zi_*( expr , u , v , T [ , t [ , t0 ] ] ) 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 54 Verilog-A Mathematical Functions 436 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 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Introduction to Verilog-A Table 54 Verilog-A Mathematical Functions (Continued) Function Description Domain Return Value 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) xy if x>=0, all y; if x<0, int(y) real floor(x) Floor all x real ceil(x) Ceiling all x real Transcendental Functions The following mathematical functions are available when using HSPICE with Verilog-A. Table 55 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 HSPICE® Simulation and Analysis User Guide X-2005.09 437 12: Using HSPICE with Verilog-A Introduction to Verilog-A Table 55 Verilog-A Transcendental Function (Continued) Function Description Domain atan2(x,y) arc-tangent of x/y all x, all y hypot(x,y) sqrt(x2 + y2) 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 AC Analysis Stimuli The The AC stimulus function produces a sinusoidal stimulus for use during a small-signal analysis: ac_stim( [ analysis_name [ , mag [ , phase ]]]) 438 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Introduction to Verilog-A 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 56 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 57 Verilog-A Analog Event Controlled Statements Function Description Initial Step Event trigger at first step of an analysis. Final Step Event trigger at last step of an analysis. Cross Zero crossing threshold detection. @(initial_step[(list_of_analyses)]) @(final_step[(list_of_analyses)]) cross(expr[,dir[,time_tol[,expr_tol]]]); HSPICE® Simulation and Analysis User Guide X-2005.09 439 12: Using HSPICE with Verilog-A Timestep and Simulator Control Table 57 Verilog-A Analog Event Controlled Statements (Continued) Function Description Timer Generatse 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 58 Verilog-A Discontinuity and Time Step Limit Functions Function Purpose 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 ) ] ; 440 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Timestep and Simulator Control System Tasks and I/O Functions System functions provide access to system-level tasks as well as access to simulator information. Table 59 Verilog-A System Tasks and I/O Functions Function Return Value $param_given Returns 1 if the parameter was overridden by a module instance parameter value assignment and 0 otherwise. $table_model Models behavior of a system by interpolating between data points that are samples of that system’s behavior. $strobe Display simulation data when the simulator has converged on a solution for all nodes using a printf() style format. $display $write $strobe(args); Open a file for writing and assign it to an associated channel. $fopen multi-channel_desc = $fopen("file"); $fclose Closes a file from a previously-opened channel(s). $fclose(multi-channel_descriptor); $fstrobe $fdisplay $fwrite Write simulation data to an opened channel(s) when the simulator has converged. Follows format for $strobe. $fstrobe(multi-channel_descriptor, "information to be written"); HSPICE® Simulation and Analysis User Guide X-2005.09 441 12: Using HSPICE with Verilog-A Timestep and Simulator Control Simulator Environment Functions The environment parameter functions return simulator environment information to the module.Return circuit ambient temperature in Kelvin. Table 60 Verilog-A Environment Parameter Functions Function Return Value Circuit temperature Return circuit ambient temperature in Kelvin. Time Return absolute time in seconds. $temperature $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 } ) 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); 442 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Simulation with Verilog-A Modules 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 (e.g., *.va or *.vams file) or Compiled Model Library file (*.cml) (Mandatory) ■ HSPICE Verilog-A feature setup options (Optional, 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 how to load Verilog-A modules into HSPICE. A module must be loaded before it can be instantiated. Verilog modules are loaded into the HSPICE simulation in one of two ways: via the .hdl command inside the HSPICE netlist or via the HSPICE commandline option – hdl. 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 the model va file only, not the model file. HSPICE® Simulation and Analysis User Guide X-2005.09 443 12: Using HSPICE with Verilog-A Loading Verilog-A Devices HSPICE .hdl Netlist Command The netlist statement allows you to declare the Verilog-A source name and path explicitly within the netlist. Syntax .hdl "filename" Example .hdl "/myhome/Verilog_A_lib/res.va" The .hdl netlist command is used to load a Verilog-A model file res.va from the directory /myhome/Verilog_A_lib. HSPICE -hdl Command-line Option The -hdl command-line option is equivalent to the .hdl command in netlists. The Verilog-A file is assumed to have a *.va extension when only a prefix is provided. One -hdloption can include one Veirlog-A file, using multple -hdl options if multiple Verilog-A files needed. Syntax -hdl name Example hspice amp.sp -hdl amp.va In this example the modules are loaded from the amp.va Verilog-A source file. Verilog-A Search Path During a simulation, HSPICE searches in the current directory for Verilog-A files. You can also provide a search path via either a command-line option or an environment variable (for example, HSP_HDL_PATH) 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. 444 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Loading Verilog-A Devices Syntax hspice -hdlpath path Example 1 hspice amp.sp -hdlpath ./my_modules When a Verilog-A file cannot be found in current working directory, HSPICE searches the directory defined by -hdlpath, in this case the relative directory ./my_modules, for it. Alternatively, you can also use the HSP_HDL_PATH environment variable to define search path for Verilog-A files. Example 2 This example assumes the csh shell is used. setenv HSP_HDL_PATH /lib_path/veriloga 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. HSPICE -vamodel Command-line Option Use the -vamodel command-line option to specify cell names for Verilog-A definitions. Syntax hspice <name> -vamodel <name2> ... The name is the cell name that uses a Verilog-A definition rather than a subcircuit definition when both exist. Each command-line -vamodel option can HSPICE® Simulation and Analysis User Guide X-2005.09 445 12: Using HSPICE with Verilog-A Loading Verilog-A Devices take no more than one name. Repeat -vamodel if multiple Verilog-A modules are defined. If a name is not specified after -vamodel, then in any case the Verilog-A definition overrides the subcircuit (whenever it is available). Verilog-A File Loading Considerations Several restrictions and issues must be considered when loading Verilog- A modules: ■ The load command (.hdl) can be placed anywhere in the top level circuit. All Verilog-A modules are loaded into the system prior to any device instantiation. ■ The .hdl statement is not allowed inside .subckt blocks. If an .hdl statement is used inside a .subckt block, the simulation exits and an error message is issued. ■ The .hdl statement is not allowed inside IF-ELSEIF-ELSE blocks. If an .hdl statement is found within a block, the simulation exits and an error message is issued. ■ 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 file has an incompatible version, the simulation exits and an error message is issued. Verilog-A Behavior in a .ALTER Analysis Verilog-A .hdl load commands can be placed in .alter statements to vary the simulation behavior. One use can be to compare multiple variations of Verilog-A modules Example For the first simulation run, HSPICE loads the module called va_amp from the amp_one.va file. In the second run, HSPICE loads the va_amp module from the amp_two.va file. * simple .alter test .hdl amp_one.va v1 1 0 10 x1 1 0 va_amp 446 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices .tran 10n 100n .alter alter1 .hdl amp_two.va .end 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 sub-circuit definition 2. Verilog-A model card 3. Verilog-A module definition 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 a Verilog-A model. HSPICE® Simulation and Analysis User Guide X-2005.09 447 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices 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 'type' of model card(s) should be the same as the Verilog-A module name. Every Verilog-A module can have one or more associated model cards. The 'type' of model card(s) is the same as the Verilog-A module name. 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 is not predefined in its associated module file, HSPICE issues a warning message and ignores the parameter. Syntax .model mname type <pname1= > <pname2= > + <pname3= > … Parameter 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. pname# Parameter name. Every parameter must be predefined in its associate 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); input in; output out; .. electrical in, out; parameter real gain=1.0; parameter real fc=100e6; 448 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices analog begin … Its associated model cards can then be: .model myamp_model va_amp gain=2 fc=200e6 .model myamp_model_2 va_amp gain=10 The instantiations of Verilog-A module va_amp can be in the following different ways: x1 x2 x3 x4 x5 n1 n3 n5 n7 n9 n2 myamp_model n4 myamp_model gain=3.0 n6 myamp_model gain=2.0 fc=150e6 n8 myamp_model_2 fc=300e6 n10 va_amp The instance x1 inherits model myamp_model parameters, i.e., gain=2, fc=200e6; Similarly, the instance x2 inherits 'fc=200e6' from model myamp_model but overrides 'gain' with the value 3.0. The instance x3 overrides all model myamp_model parameters. The instance x4 inherits parameter 'gain=10' from model myamp_model_2, and overrides parameter 'fc', which is an implicit parameter in myamp_model_2. Alternatively, the instance x5 does not use a model card and directly instantiates the Verilog-A module 'va_amp' and inherits all module va_amp default parameters, which are "gain=1" and "fc=100e6." 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 HSPICE® Simulation and Analysis User Guide X-2005.09 449 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices OPT PJF PLOT PMOS PNP R U W SP Overriding Subcircuits with Verilog-A Modules If both a sub-circuit and a Verilog-A module have the same case-insensitive name, by default, HSPICE uses the sub-circuit definition. This behavior can be changed by setting the vamodel options, either at the command line or in a .OPTION statement. The VAMODEL option works on cell-based definitions only. Instance-based overriding is not supported. Netlist Option Syntax .OPTION vamodel[=name] 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. 450 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices 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. 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> … 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 sub-circuit. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 451 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices 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 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 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. 452 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Instantiating Verilog-A Devices 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(out, in, clk); input [1:4] in; input clk; output out; electrical [1:4] in; electrical out; analog begin … Its instantiation in HSPICE could be: x1 out in1 in2 in3 in4 clk d2a In this case, the nodes in1 through in4 are mapped to ports in[1] -> in[4], respectively. The order of the vector definition is important. If the bus in VerilogA 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 HSPICE® Simulation and Analysis User Guide X-2005.09 453 12: Using HSPICE with Verilog-A Module and Parameter Name Case Sensitivity 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 a case sensitive language, 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 Module Parameters Parameters in the same module with names that differ by case only cannot be reassigned in either Verilog-A instance line or Verilog-A .MODEL cards. HSPICE issues a warning message and ignores this parameter definition. 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. 454 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Module and Parameter Name Case Sensitivity 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, etc. ■ Port current ■ Port voltage ■ Internal node voltage ■ Internal named branch current ■ Internal module variables ■ Module parameters 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. 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) HSPICE® Simulation and Analysis User Guide X-2005.09 455 12: Using HSPICE with Verilog-A Module and Parameter Name Case Sensitivity 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. 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; … 456 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Module and Parameter Name Case Sensitivity 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 on page 459. Output Internal Module Variables Verilog-A internal variables, by default, are hidden from output. HSPICE Verilog-A provides a compilation environment variable, HSP_VACOMP_OPTIONS, with –G option being set, all internal variables of Verilog-A instances become accessible. However, making all internal variables 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 -G is 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. HSPICE® Simulation and Analysis User Guide X-2005.09 457 12: Using HSPICE with Verilog-A Module and Parameter Name Case Sensitivity Output Module Parameters 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. Verilog-A Device Output Simulation Data 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. 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. 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. Verilog-A module variables are not accessible. 458 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Module and Parameter Name Case Sensitivity Using Wildcards in Verilog-A 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.*) 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. HSPICE® Simulation and Analysis User Guide X-2005.09 459 12: Using HSPICE with Verilog-A Using the Stand-alone Compiler 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. Example 1 hsp-vacomp resistor.va The Verilog-A compiler, hsp-vacomp, compiles the Verilog-A module file resistor.va, and produces a Compiled Model Library file resistor.cml in the same directory. You can include the Compiled Model Library file in the same manner as the Verilog-A file in an HSPICE netlist. 460 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Setting Environment Option for HSPICE Verilog-A Compiler 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. HSPICE® Simulation and Analysis User Guide X-2005.09 461 12: Using HSPICE with 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/1.17/users/finn/modules/lib.<arch>/amp.cml Where <arch> is one of hpux, sun, linux, etc. 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/1.17/users/finn/modules/lib.<arch> /amp.cml Deleting the Cache The cache structure is maintained unless you chooses 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. 462 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Unsupported Language Features Example To delete the default cache, from the operating system command prompt, execute rm –r ~/.hsp-model-cache Unsupported Language Features The following Verilog-A LRM 2.1 Language Features are not supported. ■ Escaped identifiers For example: real \bus+index; // Not supported ■ Derived natures described in LRM version 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 version 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 HSPICE® Simulation and Analysis User Guide X-2005.09 463 12: Using HSPICE with Verilog-A Unsupported Language Features // assigned to out_value end endmodule ■ The defparam statement as described in LRM version 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; parameter dev_temp = 27; parameter res = 50; parameter tcr = 1; analog V(n1,n2) <+ I(n1,n2)*res*tcr*($temperaturedev_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 464 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Unsupported Language Features ■ Ordered parameter lists in hierarchical instantiation as described in LRM version 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 ■ Out-of-module-references as described in the LRM version 2.1, section 7. For example: 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 HSPICE® Simulation and Analysis User Guide X-2005.09 465 12: Using HSPICE with Verilog-A Unsupported Language Features ■ Vector ports, where the port expression defining the size of a port is a parameter expression, as described in LRM version 2.1 section 7.3.1. Example: 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 ■ ‘timescale directive, as described in LRM version 2.1, section 10.1. `timescale 1ns/10ps ■ // Feature not supported The $monitor function, as described in LRM version 2.1, section 10.6. $monitor("\nEvent occurred."); // Feature not supported ■ The `default_discipline directive, as described in LRM version 2.1, section 11.1. Example 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 466 HSPICE® Simulation and Analysis User Guide X-2005.09 12: Using HSPICE with Verilog-A Known Limitations ■ Access to HSPICE primitives from a Verilog-A module, as described in LRM version 2.1, section E.2. Example 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 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"), etc., 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. HSPICE® Simulation and Analysis User Guide X-2005.09 467 12: Using HSPICE with Verilog-A Known Limitations Example if ( analysis("ac") ) begin // do something end Should be written as: if( analysis("ac", "static") ) begin // do something end The same is true for the “tran” and “noise” analysis names. 468 HSPICE® Simulation and Analysis User Guide X-2005.09 13 DC Mismatch Analysis 31 Describes the use of DCmatch analysis. Mismatch The characteristics of identically designed devices on the same piece of silicon differ slightly between each other as a result of variations in manufacturing. 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 batch-to-batch or wafer-to-wafer variations, or offsets caused by operating point differences or device degradation. Simulation Methods for Variability The Monte Carlo method is generally used for predicting variations in circuit response; however it is computationally expensive. For cases where the circuit response of interest is based on a DC solution, a method called DC mismatch (DCmatch) analysis can be used. DCmatch is related to sensitivity and noise HSPICE® Simulation and Analysis User Guide X-2005.09 469 13: DC Mismatch Analysis DCmatch Analysis analyses, and requires less time than Monte Carlo. Thus, DCmatch analysis provides an efficient technique for the approximate computation of variability in 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 variations considered are local (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 special rules). 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 Gaussian 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 Gaussian distributions. In HSPICE, the variations in model parameters are defined in a special DCmatch definition block by using expressions with parameters and functions. This approach allows for a very flexible description of the relationship between device geometry and DCmatch variation. Similar to device model parameters, the expressions must be derived from dedicated test structures for a given semiconductor technology. HSPICE runs the DCmatch analysis 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. 470 HSPICE® Simulation and Analysis User Guide X-2005.09 13: DC Mismatch Analysis DCmatch Analysis Input Syntax .DCMATCH OUTVAR <THRESHOLD=T> <FILE=string> + <PERTURBATION=P> <INTERVAL=Int> Parameter Description OUTVAR Valid node voltages, the difference between node pairs, or branch currents. 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 .DCmatch V(9) V(4,2) I(VCC) HSPICE® Simulation and Analysis User Guide X-2005.09 471 13: DC Mismatch Analysis DCmatch Analysis HSPICE reports DCmatch variations on the voltage of node 9, the voltage difference between nodes 4 and 2, and on the current through the source VCC. Example 2: .DC XVal Start=1K Stop=9K Step=1K .DCmatch V(out) Interval=3 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}. DCmatch Definition Block The variations in device characteristics are described in a special definition block separate from the model file. The block contains an entry for each device type for which the DCmatch contribution must be calculated. The syntax chosen for the DCmatch Definition block allows for future extensions to other types of variability analysis. Input Syntax .Variation .Local_Variation modelType modelName modelParam1='Expression1 for Sigma' + modelParam2='Expression2 for Sigma' .End_Local_Variation .End_Variation The variable ExpressionN for Sigma defines the DCmatch variation for the model parameter of a device with the specified modelType and modelName. The expression can be a constant, a parameter, or a function containing allowed instance parameters. The variation can be specified as a percentage of the nominal value, by adding a space and a % character after the expression. With this syntax, the specified variation is divided by 100 internally. Note that expressions that require single quotes according to standard HSPICE syntax must be on a single line. 472 HSPICE® Simulation and Analysis User Guide X-2005.09 13: DC Mismatch Analysis DCmatch Analysis Accessing Instance Parameters in Expressions for Sigma Instance parameters can be referenced to specify DCmatch variation as a function of device geometry, using the syntax E(*); for example, E(L) and E(W). Supported instance parameters are: Resistor L W M Diode L W M BJT AREA AREAB AREAC JFET L W M MOS L W M M Example .Variation .Local_Variation nmos snps20N vth0='1.234e-9/sqrt(E(W)*E(L)*E(M))' pmos snps20P u0='2.345e-6/sqrt(E(W)*E(L)*E(M))' % res rmod res =3 % .End_Local_Variation .End_Variation In this example, the nmos device has an absolute variation of model parameter vth0, dependent on the square root of the total device area. The pmos device shows a relative variation of model parameter u0, dependent on the square root of the device area. The resistor exhibits a relative variation of the parameter res. DCmatch Table Output For each output variable and sweep point, HSPICE generates a sorted table with the contributions of all the relevant devices. Each table is preceded by a header with the following information: ■ sweep or operating points for which the table is generated ■ name of the output variable ■ DC value of this output variable HSPICE® Simulation and Analysis User Guide X-2005.09 473 13: DC Mismatch Analysis DCmatch Analysis ■ values used for DCmatch options ■ number of devices which had no local variability specified ■ sigma of the specified output variables due to mismatch ■ number of devices that had local variance contributions below the threshold value and were not included in the table. The table includes the sorted device contributions in the following format: ■ 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 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 10 Devices had no Local Variability specified. Total Output Sigma = 547.77uV 4 Devices with Local Variance Contribution larger than Threshold --------------------------------------------------------------Contribution Contribution Cumulative Matched Device Sigma(V) Variance (%) Variance (%) pair Name 295.89u 29.18 29.18 1 xi82.mn1 295.66u 29.13 58.31 1 xi82.mn2 252.11u 21.18 79.49 2 xi82.mp4 247.95u 20.49 99.98 2 xi82.mp3 474 HSPICE® Simulation and Analysis User Guide X-2005.09 13: DC Mismatch Analysis DCmatch Analysis 6.49u 1.72u 658.15n 0. 14.04m 984.29u 144.36u 0. 100.00 100.00 100.00 100.00 0 0 0 0 xi82.mp5 xi82.mn7 xi82.mn6 xi82.mn8 Output From .PROBE and .MEASURE Commands The sigma of the contribution of individual devices and the total of all contributions can be output 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. The output statements are ignored if a .DCMATCH command does not exist in the netlist. Syntax for .PROBE Command A .PROBE statement in conjunction with .OPTION POST creates a graph data file that has the x-values being the sweep datapoints and the y-values being the sigma of the total output variation or the device contribution at these sweep datapoints. .PROBE DC DCmatch_total .PROBE DC DCmatch(InstanceName) This type of output is useful in conjunction with a DC sweep; for example, for plotting DCMATCH as a function of bias current, temperature, or a circuit parameter. Syntax for .MEASURE Command In .MEASURE statements, the keyword DCMATCH_TOTAL is used for the total output sigma as referenced by the output variable specified in the .DCMATCH command. The keyword DCmatch(InstanceName)is used to output the contribution sigma of the specified instance. .MEAS .MEAS .MEAS .MEAS DC DC DC DC result3 result4 result5 result6 max dcmatch_total max dcmatch(InstanceName) find dcmatch_total at=SweepValue find dcmatch(InstanceName) at=SweepValue HSPICE® Simulation and Analysis User Guide X-2005.09 475 13: DC Mismatch Analysis DCmatch Analysis In combination with other DC measures: .MEAS DC systoffset avg V(inp,inn) .MEAS DC matchoffset avg DCMATCH_TOTAL .MEAS DC maxoffset param='abs(systoffset)+3.0*matchoffset' 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. 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. 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(E(W)*E(L)*E(M)) + dmpvtwll/(E(L)*sqrt(E(W)*E(M)))’ + u0 =’dmpu0wl/sqrt(E(W)*E(L)*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. 476 HSPICE® Simulation and Analysis User Guide X-2005.09 13: DC Mismatch Analysis DCmatch Analysis 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 the sigma is calculated as 1mV. The value for dmvp0 will be defined as 1mV / sqrt ( 2 ) = 0.707mV, because two devices are involved. After simulating the same setup, HSPICE reports a contribution of 0.707mV from each device, and a total variation of sqrt ( 0.7072 + 0.7072 ) mV = 1mV. This is the same value as the original sigma from the test structure. Thus, all simulation results represent one sigma. For this example to work properly, it is crucial to know that ■ transistor pairs were measured ■ characterization results represent one sigma ■ 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 know how the individual pieces are connected when interpreting the results. Example An example netlist for running DCmatch analysis using a classic 7-transistor CMOS operational amplifier, with device sizes setup as a function of parameter k, is available in the HSPICE demo directory as: $installdir/demo/hspice/apps/opampdcm.sp 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 HSPICE® Simulation and Analysis User Guide X-2005.09 477 13: DC Mismatch Analysis Reference List mp4 net18 net031 vdda pmosbulk snps20P L='k*0.5u' W='k*4.5u' M=4 ... .variation .local_variation nmos snps20N vth0='1.234e-9/sqrt(E(W)*E(L)*E(M))' + u0='2.345e-6/sqrt(E(W)*E(L)*E(M))' % pmos snps20P vth0='1.234e-9/sqrt(E(W)*E(L)*E(M))' + u0='2.345e-6/sqrt(E(W)*E(L)*E(M))' % .end_local_variation .end_variation .dcmatch v(out) .dc k start=1 stop=4 step=0.5 .meas DC systoffset find V(pos,neg) at=2 .meas DC dcmoffset find dcmatch_total at=2 .meas DC maxoffset param='abs(systoffset)+3.0*dcmoffset' .option post ... The DCmatch analysis produces four types of output from this netlist: ■ table from operating point in the run listing ■ table from DC sweep in file opampdcm.dm0 ■ total output variation as a function of k in file opampdcm.sw0 ■ values for systematic offset, total DCmatch variation, and 3-sigma amplifier offset for k=2 in file opampdcm.sw0 Reference List 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 478 HSPICE® Simulation and Analysis User Guide X-2005.09 14 Statistical Analysis and Optimization 41 Describes how to use statistical analysis and optimization in HSPICE to analyze and optimize electrical yield. 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 uses statistical techniques and observes the effects of variations in element and model parameters. Note: HSPICE RF does not support the Worst Case, Monte Carlo, and Optimization analyses described in this chapter. ■ Analytical Model Types ■ Simulating Circuit and Model Temperatures ■ Worst Case Analysis ■ Monte Carlo Analysis ■ Worst Case and Monte Carlo Sweep Example ■ Optimization ■ Optimization Examples HSPICE® Simulation and Analysis User Guide X-2005.09 479 14: Statistical Analysis and Optimization Analytical Model Types For descriptions of individual HSPICE commands referenced in this chapter, see the HSPICE Command Reference manual. Analytical Model Types To model parametric and statistical variation in circuit behavior, use: ■ The .PARAM statement investigates the performance of a circuit as you change circuit parameters. For details about the .PARAM statement, see the HSPICE Command Reference manual. ■ Temperature Variation Analysis varies the circuit and component temperatures, and compares the circuit responses. You can study the temperature-dependent effects of the circuit, in detail. ■ Monte Carlo Analysis. If you know the statistical standard deviations of component values, use this analysis to center a design. This provides maximum process yield, and determines component tolerances. HSPICE supports Monte Carlo analysis; HSPICE RF does not. ■ Worst Case Corners Analysis (HSPICE RF does not support worst-case analysis). If you know the component value limit, use this analysis to automate quality assurance, for: ■ 480 • 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 (HSPICE only; not used in HSPICE RF). Use for cell characterization, response surface, or Taguchi analysis. See “Characterizing Cells” 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 analyses. This analysis uses ASCII file format so HSPICE can automatically generate parameter values. This analysis can replace hundreds or thousands of HSPICE simulation runs. HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Simulating Circuit and Model Temperatures Use yield analyses to modify: ■ DC operating points. ■ DC sweeps. ■ AC sweeps. ■ Transient analysis. These analyses can generate scatter plots for operating point analysis. They can also generate a family of curve plots for DC, AC, and transient analysis. Use the .MEASURE statement with yield analyses to view distributions of delay times, power, or any other characteristic described in a .MEASURE statement. Often, this is more useful than viewing a family of curves that a Monte Carlo analysis generates. HSPICE supports Monte Carlo analysis; HSPICE RF does not. When you use the .MEASURE statement, HSPICE generates a table of results in an .mt# file. You can read this file in ASCII format and you can use AvanWaves to display it. Also, if you use .MEASURE statements in a Monte Carlo or data-driven analysis (HSPICE only; HSPICE RF does not support Monte Carlo or data-driven analysis), then the HSPICE output file includes calculations for standard statistical descriptors: Mean x1 + x2 + … + xn = --------------------------------------N ( x 1 – Mean ) 2 + … ( x n – Mean ) 2 = -----------------------------------------------------------------------------N–1 Variance Sigma = Variance Average Deviation x 1 – Mean + … + x n – Mean = --------------------------------------------------------------------------N–1 Simulating Circuit and Model Temperatures Temperature affects all electrical circuits. Figure 74 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. HSPICE® Simulation and Analysis User Guide X-2005.09 481 14: Statistical Analysis and Optimization Simulating Circuit and Model Temperatures ■ Element junction temperature – each resistor, transistor, or other element generates heat so an element is hotter than the ambient temperature. ■ 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 74 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 + ∆ system + ∆ part + ∆ junction = Tjunction Ids = f ( Tjunction, Tmodel ) Every element includes a DTEMP keyword, which defines the difference between junction and ambient temperature. 482 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Simulating Circuit and Model Temperatures Example The following example uses DTEMP in a MOSFET element statement: M1 drain gate source bulk Model_name W=10u + L=1u DTEMP=+20 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 HSPICE® Simulation and Analysis User Guide X-2005.09 483 14: Statistical Analysis and Optimization Worst Case Analysis parameter to DTEMP, then use the .DC statement to sweep the parameter. The DTEMP value defaults to zero. 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 2sigma or 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, polysilicon, 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: ■ 484 XL – polysilicon CD (critical dimension of the poly layer, representing the difference between drawn and actual size). HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Worst Case Analysis ■ XWn, XWp – active CD (critical dimension of the active layer, representing the difference between drawn and actual size). ■ TOX – thickness of the gate oxide. ■ 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 61 on page 485 shows whether HSPICE adds or subtracts deviations from the average. Table 61 Sigma Deviations Type Param 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. HSPICE® Simulation and Analysis User Guide X-2005.09 485 14: Statistical Analysis and Optimization Worst Case Analysis Figure 75 is an example of data that historical records produce. Figure 75 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 76 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 76 SS Worst Case Corners Library File for a CMOS Process Model Slow Corner Skew Parameters EE Extracted Skew Parameters TT Typical Corner Skew Parameters + Gaussian FF Fast Corner Skew Parameters pop. IDS 486 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Worst Case Analysis The .LIB (library) statement, and the .INCLUDE (include file) statement, access the models and skew. The library contains parameters that 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 X-2005.09 487 14: Statistical Analysis and Optimization 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 2 µ dimension, and shrink it to 1 µ, the physical size is 0.9 µ. Τhe effective electrical size is 0.8 µ. 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 77. 488 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis Figure 77 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 489 14: Statistical Analysis and Optimization Monte Carlo Analysis Random Limit Parameter Distribution ■ Absolute variation—adds variation to the average. ■ Monte Carlo analysis randomly selects the min or max variation. The value of the MONTE analysis keyword determines how many times to perform operating point, DC sweep, AC sweep, or transient analysis. 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> <)> 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> <)> 490 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis 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. Example 2 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) HSPICE® Simulation and Analysis User Guide X-2005.09 491 14: Statistical Analysis and Optimization Monte Carlo Analysis 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 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. 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>) 492 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis .PARAM xx=LIMIT(nominal_val, abs_variation) Parameter 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 493 14: Statistical Analysis and Optimization Monte Carlo Analysis 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' Figure 78 $ +/- 20% swing Monte Carlo Distribution Gaussian Distribution Uniform Distribution Population Population Abs variation Abs variation 3 Sigma Nom_value Nom_value Rel_variation=Abs_variation/Nom_value Monte Carlo Parameter Distribution Each time you use a parameter, Monte Carlo calculates a new random variable. 494 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis 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. Monte Carlo Examples HSPICE supports Monte Carlo analysis; HSPICE RF does not. Gaussian, Uniform, and Limit Functions You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/apps/mont1.sp Figure 79 119.182 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 X-2005.09 495 14: Statistical Analysis and Optimization Monte Carlo Analysis Figure 80 Gaussian Functions MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS May 15 2003 11:41:23 MONT1_SV RGAUSS_1 115.0 110.0 105.0 100.0 VOLT [LIN] 95.0 90.0 118.375 MONT1_SV RGAUSS_1 110.0 100.0 90.0 80.9998 1.0 10.0 20.0 30.0 40.0 50.0 60.0 MONTE CARLO [LIN] 496 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis Figure 81 Limit Functions MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS May 15 2003 11:41:23 MONT1.SV0 120.0 LIMIT 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 X-2005.09 497 14: Statistical Analysis and Optimization Monte Carlo Analysis Figure 82 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. HSPICE supports Monte Carlo analysis; HSPICE RF does not. Monte Carlo sweeps the VDD supply voltage from 4.5 volts to 5.5 volts. You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/apps/mondc_a.sp ■ 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. The PHOTO parameter controls the difference between the physical gate length and the drawn gate length. Because both n-channel and p-channel transistors 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. You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/apps/rc_monte.sp 498 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis Figure 83 Monte Carlo Analysis of RC Time Constant *FILE: NOM1.SP WITH UNIFORM DISTRIBUTION May 15 2003 12:38:49 992.750N MONT1.SV0 1 900.0N VOLT [LIN] 800.0N 700.0N 600.0N 10 500.0N 9 8 400.0N 300.0N 0 200.0N 400.0N 600.0N 800.0N 1.0 7 5 26 3 1 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: ■ 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 X-2005.09 499 14: Statistical Analysis and Optimization Monte Carlo Analysis Figure 84 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. Oxide thickness control is excellent for small areas on a single wafer. Therefore, 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 linewidth 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. 500 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Monte Carlo Analysis 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 HSPICE® Simulation and Analysis User Guide X-2005.09 501 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Worst Case and Monte Carlo Sweep Example HSPICE supports Monte Carlo and worst-case analysis; HSPICE RF does not. The following example measures the delay of a pair of inverters. ■ An inverter buffers the input. ■ Another inverter loads the output. The model is prepared according to the scheme described in the previous sections: ■ The first .TRAN analysis statement sweeps from the worst-case 3-sigma slow to 3-sigma fast. ■ The second .TRAN performs 100 Monte Carlo sweeps. HSPICE Input File The HSPICE input file can contain an analysis setup section. To accelerate the simulation, .OPTION AUTOSTOP automatically stops the simulation when the .MEASURE statements achieve their target values. $ inv.sp sweep mosfet -3 sigma to +3 sigma, use measure output .option nopage nomod post autostop .tran 20p 1.0n sweep sigma -3 3 .5 .option co=132 .probe tran v(in) v(1) v(2) v(3) v(4) .param vref=2.5 .meas m_delay trig v(2) val=vref fall=1 + targ v(4) val=vref fall=1 .meas m_over max v(2,1) .meas m_under min v(3,0) .param 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 4 inv x4 4 out 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 502 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example .inc gen28.inc .end Transient Sigma Sweep Results The plot in Figure 85 shows the family of transient analysis curves for the transient sweep of the sigma parameter from -3 to +3. HSPICE then algebraically couples sigma into the skew parameters. The resulting parameters modify the actual NMOS and PMOS models. Figure 85 Sweep of Skew Parameters from -3 Sigma to +3 Sigma MONTE CARLO YIELD ESTIMATION INV.TR1 2 out 5.0 4.50 4.0 VOLT [LIN] 3.50 3.0 2.50 L 2.0 1.50 1.0 500.0N 37.6334N L 0 100.0P 200.0P 300.0P TIME [LIN] 400.0P 500.0P 550.0P To view the transient curves, plot the .MEASURE output file. The plot in Figure 86 shows the measured pair delay, and the total dissipative power, against the SIGMA parameter. HSPICE® Simulation and Analysis User Guide X-2005.09 503 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Figure 86 Sweep MOS Inverter, Pair Delay and Power: -3 Sigma to 3 Sigma * INV.SP SWEEP MOS INVERTER -3 SIGMA TO +3 SIGMA INV.MT0 M_DELAY 350.0P PARAMETER [LIN] 300.0P 250.0P 200.0P INV.MT0 M_POWER 158.445P 8.9454M 8.0M 7.0M 6.0M 5.4135M -3.0 -2.0 -1.0 0 SIGMA [LIN] 1.0 2.0 3.0 Monte Carlo Results This section evaluates the output of the Monte Carlo analysis in HSPICE. HSPICE supports Monte Carlo analysis; HSPICE RF does not. The plot in Figure 87 is a quality-control step, which plots TOX against XL (polysilicon critical dimension). Synopsys graphing software returned the cloud of points based on: ■ Setting XL as the X-axis independent variable. ■ Plotting TOX with a symbol frequency of 1. These settings plot points without connecting lines. The resulting graph demonstrates that the TOX model parameter is randomly independent of XL. 504 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Figure 87 Scatter Plot, XL and TOX PARAM [LIN] SCATTER PLOT DEMONSTRATING INDEPENDENCE OF XL AND TOX INV1.MT0 [email protected] 240.0 220.0 200.0 180.0 160.0 140.0 120.0 100.0 80.0 60.0 40.0 20.0 0 -500.0N -400.0N -200.0N 0 200.0N 400.0N 500.0N XL0POLYYC0 [LIN] The next graph (see Figure 88) is a standard scatter plot showing the measured delay for the inverter pair against the Monte Carlo index number. If a particular result looks interesting—for example, if the simulation 68 (monte carlo index = 68) produces the smallest delay—then you can read the output listing file, and 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 vtopcd: delvtop = 4.1776E-02 rshncd: rshn = 45.16 rshpcd: rshp = 166.2 m_delay = 1.7946E-10 targ= 3.4746E-10 trig= 1.6799E-10 m_power = 7.7781E-03 from= 0.0000E+00 to= 1.7946E-10 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. HSPICE® Simulation and Analysis User Guide X-2005.09 505 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Figure 88 Scatter Plot of Inverter Pair Delay SCATTER PLOT OF INVERTER PAIR DELAY INV1.MT0 M_DELAY 350.0P 300.0P 250.0P 200.0P 150.0P 100.0P 50.0P 0 1.0 20.0 40.0 60.0 80.0 100.0 INDEX (LIN) 506 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Plotting against the Monte Carlo index number does not help to center the design. To center the design: 1. Graph the various process parameters against the pair delay. This graph determines the most sensitive process variables. 2. Select the pair delay as the X-axis independent variable. 3. Set the symbol frequency to 1 to obtain the scatter plot. Figure 89 plots the expected sensitivity of the output pair delay to channel length variation (polysilicon variation). Figure 89 Sensitivity of Delay with Poly CD (XL) SCATTER PLOT OF INVERTER PAIR DELAY INV1.MT0 M_DELAY 350.0P 300.0P 250.0P 200.0P 150.0P 100.0P 50.0P 0 1.0 20.0 40.0 60.0 80.0 100.0 INDEX (LIN) The next plot shows the TOX parameter against the pair delay (Figure 90). The scatter plot does not have a clear tilt, because TOX is a secondary process parameter compared to XL. To explore this in more detail, set the XL skew parameter to a constant and run a simulation. HSPICE® Simulation and Analysis User Guide X-2005.09 507 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Figure 90 Sensitivity of Delay with TOX SENSITIVITY OF PAIR DELAY WITH RESPECT TO TOX INV1.MT0 [email protected] 240.0 PARAM [LIN] 220.0 200.0 180.0 160.0 140.0 120.0 100.0 100.0P 150.0P 200.0P 250.0P 300.0P 350.0P M_DELAY (LIN) The plot in Figure 91 overlays a 3-sigma, worst-case corners response on a 100-point Monte Carlo analysis. The actual (Monte Carlo) distribution for power/delay is very different from the +3 sigma to -3 sigma plot. ■ This example simulated the worst case in 0.5 sigma steps. ■ The actual response is closer to ± 1.5 sigma instead of ± 3 sigma. ■ This produces a predicted delay variation of 100 ps instead of 200 ps. Therefore, the advantage of using Monte Carlo over traditional 3-sigma, worstcase corners is a 100% improvement in accuracy of simulated-to-actual distribution. This shows how the worst-case procedure is overly pessimistic. 508 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Worst Case and Monte Carlo Sweep Example Figure 91 Superimposing Sigma Sweep Over Monte Carlo SUPERIMPOSE +3 SIGMA TO -3 SIGMA SWEEP OVER MONTE CARLO INV1.MT0 M_POWER INV.MT0 M_POWER 10.0M 9.50M +3 sigma PARAM [LIN] 9.0M 8.50M 8.0M 7.50M 7.0M 6.50M -3 sigma 6.0M 5.50M 5.0M 100.0P.0 150.0P 200.0P 250.0P M_DELAY (LIN) 300.0P 350.0P 400.0P Figure 92 superimposes the assumed part grades from marketing studies onto the Monte Carlo plot. This example uses a 250 ps delay and 7.5 mW power dissipation to determine the four binning grades. A manual count shows: ■ Bin1 - 13% ■ Bin2 - 37% ■ Bin3 - 27% ■ Bin4 - 23% If this circuit is representative of the entire chip, then the present yield should be 13% for the premium Bin 1 parts, assuming variations in design and process. HSPICE® Simulation and Analysis User Guide X-2005.09 509 14: Statistical Analysis and Optimization Optimization Figure 92 Speed/Power Yield Estimation MONTE CARLO YIELD ESTIMATION 9.0M 8.750M PARAM [LIN] 8.50M 8.250M INv1.MT0 M_POWER Bin 2 - 37 sims Bin 4 - 23 sims 8.0M 7.750M 7.50M 7.250M 7.0M 6.750M 6.50M 6.250M 6.0M 150.0P Bin 1 - 13 sims 200.0P 250.0P M_DELAY (LIN) Bin3 - 27 sims 300.0P 350.0P Optimization 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 manual 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. 510 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 511 14: Statistical Analysis and Optimization Optimization 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 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. 512 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization 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. 1. To specify goal optimizations, 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 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. HSPICE® Simulation and Analysis User Guide X-2005.09 513 14: Statistical Analysis and Optimization Optimization Optimization 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. 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: 1. Analysis statement with OPTIMIZE. 2. .MEASURE statements specifying optimization goals or error functions. 3. Ordinary analysis statement. 4. Output statements. 514 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples 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 Parameter 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. 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 HSPICE® Simulation and Analysis User Guide X-2005.09 515 14: Statistical Analysis and Optimization Optimization Examples ■ 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: ■ VTO ■ GAMMA ■ UO ■ VMAX ■ 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: 516 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples ■ 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. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 517 14: Statistical Analysis and Optimization Optimization Examples 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 93 shows the results. Figure 93 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 0 1.0 1.50 2.0 2.5 3.0 YOS [LIN] 3.5 4.0 4.50 5.0 OPTLEVELS.90 IM ANP [LIN] 5.0M 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. 518 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples 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 94 on page 519 shows the results. DC Optimization Input Netlist File for Level 13 Model You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/mos/ml13opt.sp Figure 94 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] HSPICE® Simulation and Analysis User Guide X-2005.09 3.0 4.0 5.0 519 14: Statistical Analysis and Optimization Optimization Examples 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: ■ 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. 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 You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/ciropt/rcopt.sp Optimization Results RESIDUAL SUM OF SQUARES NORM OF THE GRADIENT MARQUARDT SCALING PARAMETER NO. OF FUNCTION EVALUATIONS NO. OF ITERATIONS = 9 520 = = = = 4.291583E-16 5.083346E-04 2.297208E-04 20 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples Residual Sum of Squares The residual sum of squares is a measure of the total error. The smaller this value is the more accurate the optimization results are. ne residual sum of squares = ∑ Ei 2 i=1 In this equation, E is the error function, and ne is the number of error functions. Norm of the Gradient The norm of the gradient is another measure of the total error. The smaller this value is the more accurate the optimization results are. The following equations calculates the G gradient: ne Gj = ∑ E i ⋅ ( ∆E i ⁄ ∆P j ) i=1 np norm of the gradient = 2 ⋅ ∑ Gj 2 i=1 In this equation, P is the parameter, and np is the number of parameters to optimize. Marquardt Scaling Parameter The Levenburg-Marquardt algorithm uses this parameter to find the actual solution for the optimizing parameters. The search direction is a combination of the Steepest Descent method and the Gauss-Newton method. 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. HSPICE® Simulation and Analysis User Guide X-2005.09 521 14: Statistical Analysis and Optimization Optimization Examples 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 $ Figure 95 55.6965 5.7945m 44.3035 5.1872m 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 522 0 200.0M 400.0M 600.0M TIME [LIN] 800.0M 1.0 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples Figure 96 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: 1. Rising edge delay of 5 ns (input 50% voltage to output 50% voltage). 2. Falling edge delay of 5 ns (input 50% voltage to output 50% voltage). 3. RMS power dissipation should be as low as possible. 4. 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 X-2005.09 523 14: Statistical Analysis and Optimization Optimization Examples ■ 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 You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/apps/trist_buf_opt.sp Figure 97 Tristate Buffer Optimization Circuit g VCC p VCC VCC MP1 VCC VCC VCC MP3 MP2 DATAN BUS MN1 Cbus MN2 PEN MP11 MP10 NENN MP5 MN3 MN12 MP12 VCC PENN MP4 Cext Cpad MN10 MN11 NEN MN5 MN4 ENB VCC MP13 ENBN Cenb 524 Cenbn MN13 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples Figure 98 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 ASIC2.TR0 OUT 4.0 OUTBAR VOLT [LIN] 3.50 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 X-2005.09 525 14: Statistical Analysis and Optimization Optimization Examples 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 NORM OF THE GRADIENT MARQUARDT SCALING PARAMETER CO. OF FUNCTION EVALUATIONS NO. OF ITERATIONS = = = = = 5.142639e-02 6.068882e-02 0.340303 170 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 526 HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples Figure 99 BJT-S Parameter Optimization FILE: BJTOPT.SP NETWORK S-PARAMETER OPTIMIZATION APRIL 22, 2004 6:22:34 BJTOPT.AC0 20.0 10.0 1.9879 BJTOPT.AC0 650.0N [LIN] 600.0N 550.0N BJTOPT.AC0 500.0N 450.0N 400.0N 96.8250N BJTOPT.AC0 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 X-2005.09 527 14: Statistical Analysis and Optimization Optimization Examples 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 100 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 528 400.0M 500.0M 600.0M BASEF [LIN] 700.0M 800.0M 820.0M HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples Figure 101 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 X-2005.09 529 14: Statistical Analysis and Optimization Optimization Examples GaAsFET Model DC Optimization Input Netlist File You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/devopt/jopt.sp Figure 102 JFET Optimization *FILE: JOPT.SP JFET OPTIMIZATION APRIL 22, 2004 18:41:12 JOPT.SVO 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: 530 ■ 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. HSPICE® Simulation and Analysis User Guide X-2005.09 14: Statistical Analysis and Optimization Optimization Examples 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. ■ Calculate the transistor area algebraically use a voltage value and minimize the resulting voltage. ■ The transistor area measure statement uses MINVAL, which assigns less weight to the area minimization. ■ Optimizes the bias voltage. MOS Op-amp Optimization Input Netlist File You can find the sample netlist for this example in the following directory: $installdir/demo/hspice/ciropt/ampopt.sp Figure 103 CMOS Op-amp vsupply M4 M3 M6 vout vin- M1 vbias M2 vin+ M5 M7 HSPICE® Simulation and Analysis User Guide X-2005.09 531 14: Statistical Analysis and Optimization Optimization Examples Figure 104 Operational Amplifier Optimization AMPORT.SP MOS OPERATIONAL AMPLIFIER OPTIMIZATION APRIL 22, 2004 18:57:06 3.9877 AMPORT.TR0 3.0 VOLT [LIN] 2.0 1.0 AMPORT.TR0 POWER 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] 532 HSPICE® Simulation and Analysis User Guide X-2005.09 15 Running Demonstration Files 51 Contains examples of basic file construction techniques, advanced features, and simulation tricks. Lists and describes several HSPICE and HSPICE RF input files. This chapter includes the following topics: ■ Using the Demo Directory Tree ■ Two-Bit Adder Demo ■ MOS I-V and C-V Plotting Demo ■ CMOS Output Driver Demo ■ Temperature Coefficients Demo ■ Simulating Electrical Measurements ■ Modeling Wide-Channel MOS Transistors ■ Demonstration Input Files HSPICE® Simulation and Analysis User Guide X-2005.09 533 15: Running Demonstration Files Using the Demo Directory Tree Using the Demo Directory Tree Demonstration Input Files on page 552 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: 534 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 /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 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Two-Bit Adder Demo 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. Figure 105 One-bit Adder sub-circuit in1 1 X8 X2 in2 X4 X7 10 13 X5 X1 half1 2 X8 4 TIME [LIN] X3 9 carry-in X6 #1_nand HSPICE® Simulation and Analysis User Guide X-2005.09 out half2 carry-out X9 535 15: Running Demonstration Files MOS I-V and C-V Plotting Demo Figure 106 Two-bit Adder Circuit A(0) B(0) A(1) B(1) carry-out_1 carry-in One Bit One Bit C(0) C(1) carry-out_2 Figure 107 1-bit NAND Gate Binary Adder in1 1 X8 X2 in2 X4 X7 10 13 X5 X1 half1 2 X8 4 TIME [LIN] X3 9 carry-in X6 #1_nand out half2 carry-out 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 536 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files MOS I-V and C-V Plotting Demo shows how to easily create input files, and how to display the complete graphical results. The following features aid model evaluations: Table 62 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. 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 63 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 X-2005.09 537 15: Running Demonstration Files MOS I-V and C-V Plotting Demo Figure 108 MOS IDS Plot *FILE: MOS2BJT.SP TR0 BJT MOS ADDER APRIL 24, 2003 13:12:24 4.50 MOS2BJT.TR0 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] 538 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files MOS I-V and C-V Plotting Demo Figure 109 MOS VGS Plot *FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOT APRIL 24, 2003 14:18:58 MOS1VGS.SV0 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 X-2005.09 4.0 5.0 539 15: Running Demonstration Files MOS I-V and C-V Plotting Demo Figure 110 MOS GM Plot *FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS APRIL 24, 2003 14:31:48 59.5887U MOS1VGS.SV0 55.0U 50.0U 45.0U AMP [LIN] 40.0U 35.0U 30.0U 25.0U 20.0U 15.0U 10.0U 5.0U 0 540 0 1.0 2.0 3.0 VOLTS [LIN] 4.0 5.0 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files CMOS Output Driver Demo Figure 111 MOS C-V Plot *FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS APRIL 24, 2003 14:42:16 13.7840F MOS1VGS.SV0 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 X-2005.09 541 15: 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: 542 ■ Create a five-lump transmission line model for the copper wire. ■ Create single lumped models for leadframe loads. HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files CMOS Output Driver Demo Figure 112 Noise Bounce *FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS APRIL 24, 2004 14:53:29 MOS1VGS.SV0 59.5887U GM_N 55.0U GM_P 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 X-2005.09 543 15: Running Demonstration Files CMOS Output Driver Demo Figure 113 Asic1.sp Demo Local Supply Voltage *FILE: MOS1VGS.SP IDS, VGS,CV, AND GM PLOTS APRIL 24, 2003 15:24:31 13.7840F MOS1VGS.SV0 CG-TOT_N 13.0F CG-TOT_P LX [LIN] 12.0F 11.0F 10.0F 9.0F 8.0F 7.0F 6.0F 0 544 1.0 2.0 3.0 VOLTS [LIN] 4.0 5.0 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files CMOS Output Driver Demo Figure 114 Asic1.sp Demo Local Supply Current *FILE: ASIC1.SP GROUND BOUNCE FOR I/O CMOS DRIVER APRIL 24, 2003 15:29:24 5.8829 ASIC1.TR0 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 X-2005.09 545 15: Running Demonstration Files Temperature Coefficients Demo Figure 115 Asic1.sp Demo Input and Output Signals *FILE: ASIC1.SP GROUND BOUNCE FOR I/O CMOS DRIVER APRIL 24, 2004 15:39:18 ASIC1.TR0 POWER 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 20.0N 25.0N 30.0N TIME [LIN] 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. 546 HSPICE® Simulation and Analysis User Guide X-2005.09 15: 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 X-2005.09 547 15: 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: 548 ■ TURN ONfrom 90% of input rising, to 90% of output falling. ■ OUTPUT FALLfrom 90% to 10% of output falling. ■ TURN OFFfrom 10% of input falling, to 10% of output rising. ■ OUTPUT RISEfrom 10% to 90% of output rising. HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Modeling Wide-Channel MOS Transistors Figure 116 T2N2222 Optimization *FILE: ASIC2.SP TEST OF I/O STAGE LUMPED MOS MODEL APRIL 24, 2003 15:52:09 ASIC2.TR0 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 X-2005.09 549 15: 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. 550 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Modeling Wide-Channel MOS Transistors Figure 117 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: $installdir/demo/hspice/apps/asic3.sp HSPICE® Simulation and Analysis User Guide X-2005.09 551 15: Running Demonstration Files Demonstration Input Files Figure 118 Asic3 Single vs. Lumped Model *FILE: ASIC2.SP TEST OF I/O STAGE LUMPED MOS MODEL APRIL 24, 2004 16:02:35 ASIC2.TR0 10.0M 9.0M 8.0M PARAM [LIN] 7.0M 6.0M 5.0M 4.0M 3.0M 2.0M 1.0M 0 -1.0M 0 200.0 400.0 600.0 800.0 TIME [LIN] Demonstration Input Files File Name Description Algebraic Output Variable Examples$installdir/demo/hspice/alge 552 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 X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description xalg2.sp QA of parameters Applications of General Interest$installdir/demo/hspice/apps alm124.sp AC, noise, and transient op-amp analysis alter2.sp .ALTER examples ampg.sp pole/zero analysis of a G source amplifier asic1.sp ground bounce for I/O CMOS driver asic3.sp ten-stage lumped MOS model bjt2bit.sp BJT two-bit adder bjt4bit.sp four-bit all NAND gate, binary adder bjtdiff.sp BJT diff amp with every analysis type bjtschmt.sp bipolar Schmidt trigger bjtsense.sp bipolar sense amplifier cellchar.sp characteristics of ASIC inverter cell crystal.sp crystal oscillator circuit gaasamp.sp simple GaAsFET amplifier grouptim.sp group time-delay example inv.sp sweep MOSFET -3 sigma to +3 sigma use .MEASURE output mcdiff.sp CMOS differential amplifier mondc_a.sp Monte Carlo of MOS diffusion and photolithographic effects (HSPICE only) mondc_b.sp Monte Carlo DC analysis (HSPICE only) mont1.sp Monte Carlo Gaussian, uniform, and limit function (HSPICE only) HSPICE® Simulation and Analysis User Guide X-2005.09 553 15: Running Demonstration Files Demonstration Input Files File Name Description mos2bit.sp two-bit MOS adder opampdcm.sp DCmatch analysis pll.sp phase-locked loop sclopass.sp switched-capacitor low-pass filter worst.sp worst case skew models by using .ALTER xbjt2bit.sp BJT NAND gate two-bit binary adder Behavioral Applications$installdir/demo/hspice/behave 554 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 X-2005.09 15: 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$installdir/demo/hspice/bench bigmos1.sp large MOS simulation demo.sp quick demo file to test installation m2bit.sp 72-transistor two-bit adder – typical cell simulation m2bitf.sp fast simulation example HSPICE® Simulation and Analysis User Guide X-2005.09 555 15: Running Demonstration Files Demonstration Input Files File Name Description m2bitsw.sp Fast simulation example. Same as m2bitf.sp, but uses behavioral elements senseamp.sp bipolar analog test case Timing Analysis$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 556 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 X-2005.09 15: 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 X-2005.09 557 15: Running Demonstration Files Demonstration Input Files File Name Description alf353.sp characteristics of National wide-bandwidth, dual JFET input, opamp 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 558 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 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description alm258a.sp characteristics of National op-amp 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 op-amp amc1741.sp characteristics of Motorola internally-compensated, highperformance op-amp HSPICE® Simulation and Analysis User Guide X-2005.09 559 15: Running Demonstration Files Demonstration Input Files 560 File Name Description amc1747.sp characteristics of Motorola internally-compensated, highperformance op-amp 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 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description j2n3330.sp characteristics of JFET 2n3330 I-V mirf340.sp characteristics of IRF340 I-V t2n2222.sp characteristics of BJT 2n2222 Device Optimization (HSPICE only)$installdir/demo/hspice/devopt beta.sp LEVEL=2 beta optimization bjtopt.sp s-parameter optimization of a 2n6604 BJT bjtopt1.sp 2n2222 DC optimization bjtopt2.sp 2n2222 Hfe optimization d.sp diode, multiple temperatures dcopt1.sp 1n3019 diode, I-V and C-V optimization gaas.sp JFET optimization jopt.sp 300u/1u GaAs FET, DC optimization jopt2.sp JFET optimization joptac.sp 300u/1u GaAs FET, 40 MHz–20 GHz, s-parameter optimization l3.sp MOS LEVEL 3 optimization l3a.sp MOS LEVEL 3 optimization l28.sp LEVEL=28 optimization ml2opt.sp MOS LEVEL=2 I-V optimization ml3opt.sp MOS LEVEL=3 I-V optimization ml6opt.sp MOS LEVEL=6 I-V optimization ml13opt.sp MOS LEVEL=13 I-V optimization HSPICE® Simulation and Analysis User Guide X-2005.09 561 15: Running Demonstration Files Demonstration Input Files File Name Description opt_bjt.sp 2n3947 forward and reverse Gummel optimization Fourier Analysis (HSPICE only)$installdir/demo/hspice/fft 562 am.sp FFT analysis, AM source 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 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description kaiser.sp FFT analysis, Kaiser window mod.sp FFT analysis, modulated pulse pulse.sp FFT analysis, pulse source 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$installdir/demo/hspice/filters fbp_1.sp bandpass LCR filter, measurement fbp_2.sp bandpass LCR filter, pole/zero fbpnet.sp bandpass LCR filter, s-parameters fbprlc.sp LCR AC analysis for resonance fhp4th.sp high-pass LCR, fourth-order Butterworth filter fkerwin.sp pole/zero analysis of Kerwin’s circuit flp5th.sp low-pass, fifth-order filter flp9th.sp low-pass, ninth-order FNDR, with ideal op-amps HSPICE® Simulation and Analysis User Guide X-2005.09 563 15: Running Demonstration Files Demonstration Input Files File Name Description micro1.sp test of microstrip micro2.sp test of microstrip tcoax.sp test of RG58/AU coax trans1m.sp FR-4, printed-circuit, lumped transmission line Magnetics$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$installdir/demo/hspice/mos 564 bsim3.sp LEVEL=47 BSIM3 model cap13.sp plot MOS capacitances, LEVEL=13 model cap_b.sp capacitances for LEVEL=13 model cap_m.sp capacitance for LEVEL=13 model capop0.sp plot MOS capacitances, LEVEL=2 capop1.sp plot MOS capacitances, LEVEL=2 capop2.sp plot MOS capacitances, LEVEL=2 capop4.sp plot MOS capacitances, LEVEL=6 chrgpump.sp charge-conservation test, LEVEL=3 iiplot.sp plot of impact ionization current ml6fex.sp plot temperature effects, LEVEL=6 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description ml13fex.sp plot temperature effects, LEVEL=13 ml13ft.sp s-parameters for LEVEL=13 ml13iv.sp plot I-V for LEVEL=13 ml27iv.sp plot I-V for LEVEL=27 SOSFET mosiv.sp plot I-V for files that you include mosivcv.sp plot I-V and C-V for LEVEL=3 qpulse.sp charge-conservation test, LEVEL=6 qswitch.sp charge-conservation test, LEVEL=6 selector.sp automatic model selector for width and length tgam2.sp LEVEL=6, gamma model tmos34.sp MOS LEVEL=34 EPFL, test DC Radiation Effects$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 HSPICE® Simulation and Analysis User Guide X-2005.09 565 15: Running Demonstration Files Demonstration Input Files 566 File Name Description drad6.sp example of diode radiation effects dradarb2.sp example of diode radiation effects jex1.sp example of JFET radiation effects 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 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description 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) 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 voltage-divider rad13.sp three-input NMOS NAND gate with non-EPI, EPI and SOS examples rad14.sp GaAs differential-amplifier circuit rad14dc.sp n-channel JFET, DC I-V curves Sources$installdir/demo/hspice/sources amsrc.sp amplitude modulation exp.sp exponential independent source pulse.sp test of pulse pwl.sp repeated piecewise-linear source pwl10.sp op-amp, voltage follower rtest.sp voltage-controlled resistor, inverter chain sffm.sp single-frequency, FM modulation source sin.sp sinusoidal source, waveform vcr1.sp switched-capacitor network by using G-switch HSPICE® Simulation and Analysis User Guide X-2005.09 567 15: Running Demonstration Files Demonstration Input Files File Name Description Transmission Lines$installdir/demo/hspice/tline 568 fr4.sp microstrip test, FR-4 PC board material fr4o.sp optimizing model for microstrip FR-4 PC board material 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 HSPICE® Simulation and Analysis User Guide X-2005.09 15: Running Demonstration Files Demonstration Input Files File Name Description Verilog-A$installdir/demo/hspice/veriloga resistor.sp a very simple Verilog-A resistor model sinev.sp simple voltage source 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 X-2005.09 569 15: Running Demonstration Files Demonstration Input Files 570 HSPICE® Simulation and Analysis User Guide X-2005.09 A Full Simulation Examples A 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 Cosmos-Scope. Simulation Example Using AvanWaves Input Netlist and Circuit The following 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 Rinterm in gnd 51 HSPICE® Simulation and Analysis User Guide X-2005.09 571 A: Full Simulation Examples Simulation Example Using AvanWaves 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 You can find the complete sample netlist for this example in the following directory: $installdir/demo/hspice/bench/example.sp Figure 119 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). 572 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using AvanWaves Figure 119 Circuit Diagram for Linear CMOS Inverter Analog Source 10 MHz 1V to 5V +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 64 HSPICE Output Files File Name 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 X-2005.09 573 A: 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: lic: lic: lic: 574 Using FLEXlm license file: /afs/rtp/product/distrib/bin/license/license.dat Checkout hspice; Encryption code: AC34CE559E01F6E05809 License/Maintenance for hspice will expire on 14-apr- HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using AvanWaves + 1999/1999.200 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 +0:clamp = 2.6200 0:in = 0. +0:inv1out =2.6200 0:inv2out = 2.6199 node =voltage 0:infilt = 2.6200 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 ***** HSPICE® Simulation and Analysis User Guide X-2005.09 575 A: Full Simulation Examples Simulation Example Using AvanWaves falltime= 1.5645E-08 targ= 5.7994E-08 trig= 4.2348E-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 = 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-08 576 trig= 4.7072E-08 HSPICE® Simulation and Analysis User Guide X-2005.09 A: 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 = analysis time # points op point 0.04 1 transient 4.71 505 readin 0.03 errchk 0.01 setup 0.01 output 0.01 0 # jfets = 0 # mosfets = 4 tot. iter conv.iter 23 9322 2624 rev= 664 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 HSPICE® Simulation and Analysis User Guide X-2005.09 577 A: Full Simulation Examples Simulation Example Using AvanWaves lic: License/Maintenance for hspice will expire on + 14-apr-1999/1999.200 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= + cpu clock= 2.83E+00 tran: time= 1.01016E-07 tot_iter= 186 conv_iter= tran: time= 2.02642E-07 tot_iter= 338 conv_iter= tran: time= 3.01763E-07 tot_iter= 495 conv_iter= tran: time= 4.04254E-07 tot_iter= 668 conv_iter= 578 101 54 98 145 198 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using AvanWaves tran: tran: tran: tran: tran: tran: time= time= time= time= time= time= 5.02594E-07 6.10102E-07 7.01850E-07 8.01776E-07 9.04268E-07 1.00000E-06 tot_iter= tot_iter= tot_iter= tot_iter= tot_iter= tot_iter= 841 983 1161 1306 1481 1654 conv_iter= 248 conv_iter= 289 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 HSPICE® Simulation and Analysis User Guide X-2005.09 579 A: Full Simulation Examples Simulation Example Using AvanWaves dcop: end dcop, cpu clock= 5.84E+00 memory= 155 kb + 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 120 through Figure 125 show the six different postprocessor outputs from the simulation of the example netlist. These plots are postscript output from the actual data in AvanWaves, a Synopsys graphical waveform viewer. 580 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using AvanWaves HSPICE® Simulation and Analysis User Guide X-2005.09 581 A: Full Simulation Examples Simulation Example Using AvanWaves Figure 120 Plot of Voltage on Node in example HSPICE netlist using a linear CMOS amplifier 5 4.5 4 3.5 3 2.5 2 1.5 Voltages 1 650m 0 -650m -1 -1.5 -2 -2.5 -3 -3.5 -4 -4.5 -5 582 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using AvanWaves Figure 121 Plot of Voltage on Node clamp vs. Time example HSPICE netlist using a linear CMOS amplifier 6 5.5 5 4.5 4 3.5 Voltages 3 2.5 2 1.5 1 500m 0 -500m -50n 0 50n 250n 150n 300n 350n400n 450n500n 550n600n 650n700n 750n 200n 100n 800n 850n900n 950n HSPICE® Simulation and Analysis User Guide X-2005.09 583 A: Full Simulation Examples Simulation Example Using AvanWaves Figure 122 Plot of Voltage on Node inv1out vs.Time Voltages example HSPICE netlist using a linear CMOS amplifier 5.2 5 4.8 4.6 4.4 4.2 4 3.8 3.6 3.4 3.2 3 2.8 2.6 2.4 2.2 2 1.8 1.6 1.4 1.2 1 800m 600m 400m 200m 0 -200m 0 -50n 584 250n 150n 50n 300n 350n 400n 450n500n 550n600n 650n700n 750n 100n 200n 800n 850n HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using AvanWaves Figure 123 Plot of Voltage on Node inv2out vs. Time Voltages example HSPICE netlist using a linear CMOS amplifier 5.2 5 4.8 4.6 4.4 4.2 4 3.8 3.6 3.4 3.2 3 2.8 2.6 2.4 2.2 2 1.8 1.6 1.4 1.2 1 800m 600m 400m 200m 0 -200m 800n 700n 300n 1000n 900n 500n 600n 400n 200n 750n 950n 850n 650n -50n 0 50n 100n150n 350n 550n 450n 250n HSPICE® Simulation and Analysis User Guide X-2005.09 585 A: Full Simulation Examples Simulation Example Using AvanWaves Figure 124 Plot of Current through Diode dlow vs. Time example HSPICE netlist using a linear CMOS amplifier 17m 16m 15m 14m 13m 12m 11m Currents 10m 9m 8m 7m 6m 5m 4m 3m 2m 1m 0 800n 700n 300n 900n 1000n 500n 600n 400n 200n 750n 950n 850n 650n -50n 0 50n 100n150n 350n 550n 450n 250n 586 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using Cosmos-Scope Figure 125 Plot of Measured Variable falltime vs. Amplifier Input Voltage example HSPICE netlist using a linear CMOS amplifier 40n 38n 36n 34n 32n 30n 28n Measure 26n 24n 22n 20n 18n 16n 14n 12n 10n 8n 6n 800m 1 1.2 1.4 1.6 1.8 2 2.2 2.4 2.6 2.8 3 3.2 3.4 3.6 3.8 4 4.2 4.4 4.6 4.8 5 Simulation Example Using Cosmos-Scope 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 The following example of an HSPICE netlist shows the input netlist for a BJT diff amplifier. Comment lines indicate the individual sections of the netlists. See the HSPICE Command Reference manual for information about individual commands. HSPICE® Simulation and Analysis User Guide X-2005.09 587 A: Full Simulation Examples Simulation Example Using Cosmos-Scope *file: bjtdiff.sp bjt diff amp with every analysis type *# ANALYSIS: ac dc tran tf noise new four sens pz disto temp *# OPTIONS: list node ingold=2 measdgt=5 numdgt=8 + probe post *# TEMPERATURE: 25 * netlist options .OPTION list node ingold=2 measdgt=6 numdgt=8 probe post * defined parameters .PARAM rb1x=aunif(20k,1k,30k) rb2x=aunif(20k,1k,30k) * analysis specifications .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 .DISTRO rc1 20 .9 1m 1.0 .SENS v(4) .TRAN 5ns 200ns .FOUR 5meg v(5) v(15) .TEMP -55 150 * output specifications .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 .PROBE dc v(4) v(5) v(14) v(15) .PROBE ac vm(5) vp(5) vm(15) vp(15) .PROBE ac vt(5) vt(15) .PROBE noise onoise(m) inoise(m) .PROBE ac z11(m) z12(m) z22(m) zin(m) .PROBE disto hd2 hd3 sim2 dim2 dim3 .PROBE tran v(4) v(5) v(14) v(15) .PROBE tran p(vcc) p(vee) p(vin) power * source statements VIN 1 0 sin(0 0.1 5meg) ac 1 VCC 8 0 12 VEE 9 0 -12 * circuit statements q1 4 2 6 qnl q11 14 12 16 qpl q2 5 3 6 qnl q21 15 13 16 qpl rs1 1 2 1k 588 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using Cosmos-Scope rs11 1 12 1k rs2 3 0 1k rs12 13 0 1k rc1 4 8 10k 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 definitions .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 You can find the complete sample netlist for this example in the following directory: $installdir/demo/hspice/apps/bjtdiff.sp 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. HSPICE® Simulation and Analysis User Guide X-2005.09 589 A: Full Simulation Examples Simulation Example Using Cosmos-Scope Simulation creates the following output files: Table 65 Output Files File Name 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 Cosmos-Scope The steps below show how to use the Synopsys Cosmos-Scope 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 1. Invoke Cosmos-Scope. From a Unix command line, type: % cscope On a Windows-NT system, choose the menu command: Programs > (user_install_location)> Cosmos-Scope 2. Open the Open Plotfiles dialog box: File > Open > Plotfiles 3. In the Open Plotfiles dialog box, in the Files of Type fields, select the Hspice Transient (*.tr*) item. 590 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using Cosmos-Scope 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 126 on page 592. HSPICE® Simulation and Analysis User Guide X-2005.09 591 A: Full Simulation Examples Simulation Example Using Cosmos-Scope Figure 126 Transient Analysis: Plot of v(4), v(5), and ITPOWERD (power) Graph1 8.0 (TPOWRD)>t(s) 0.1208 (v):t(s) v(4) 0.1207 7.0 v(5) 0.1206 (V) 6.0 5.0 (TPOWRD) 0.1205 0.1204 0.1203 0.1202 4.0 0.1201 0.12 3.0 0.1199 0.0 25n 50n 75n 100n 125n t(s) 150n 175n 200n 225n Viewing HSPICE AC Analysis Waveforms 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. 592 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using Cosmos-Scope 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 127. Figure 127 AC Analysis Result: Plot of dim2(mag), dim3(mag) from bjtdiff.ac0 0.071 (DIM2):Frequency(Hertz) Graph2 0.02 dim2(meg) 0.07075 0.018 Frequency (Hertz dim3(meg) 0.0705 (DIM3):Frequency (Hertz) 0.016 0.07025 0.014 0.07 0.012 0.06975 0.01 0.0695 0.008 0.06925 0.006 0.069 0.06875 0.004 0.0685 0.002 0.0 0.0 (DIM2) (DIM3) 0.06825 1meg 2meg 3meg 4meg 5meg 6meg Frequency (Hertz) HSPICE® Simulation and Analysis User Guide X-2005.09 7meg 8meg 9meg 10meg 593 A: Full Simulation Examples Simulation Example Using Cosmos-Scope Viewing HSPICE DC Analysis Waveforms 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 128 on page 595. 594 HSPICE® Simulation and Analysis User Guide X-2005.09 A: Full Simulation Examples Simulation Example Using Cosmos-Scope Figure 128 DC Analysis Result: Plot of v(14), v(15), v(4), and v(5) from bjtdiff.sw0 (V): Voltage K(Volt) v(14) Graph3 15.0 v(15) v(4) 10.0 v(5) (V) 5.0 0.0 -5.0 -10.0 -15.0 -0.25 -0.2 -0.15 -0.1 -0.05 0.0 0.05 Voltages K(volt) 0.1 0.15 0.2 0.25 The Cosmos-Scope 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 HSPICE® Simulation and Analysis User Guide X-2005.09 595 A: Full Simulation Examples Simulation Example Using Cosmos-Scope 596 HSPICE® Simulation and Analysis User Guide X-2005.09 Index Symbols !GND node 54 $installdir installation directory 67 A A2D function 200 model parameter 200 output model parameters 204 See also mixed mode .a2d file 16, 18, 200 ABS element parameter 196 abs(x) function 228 ABSI option 327 ABSMOS option 327 absolute power function 228 value function 228 value parameter 196 ABSV option 327 ABSVAR option 356 AC analysis 243 output 260 RC network 382 resistance 381 small signals 380 sources 130 AC analysis measurement results file 17 AC analysis results file 17 .AC statement 483, 515 .ac# file 16, 17 accuracy control options 328 simulation time 327 tolerance 325, 326, 354 ACCURATE option 356 HSPICE® Simulation and Analysis User Guide X-2005.09 ACM model parameter 356 acos(x) function 227 ACOUT option 262–263 adder circuit 536 demo 535 NAND gate binary 536 subcircuit 535 admittance AC input 266 AC output 266 Y parameters 260 AF model parameter 386 AGAUSS keyword 493 algebraic expressions 226 models 356 algorithm linear acceleration 358 numerical integration 366 algorithms Damped Pseudo Transient algorithm 335 DVDT 367, 368 GEAR 363 integration 363 iteration count 367 Levenberg-Marquardt 521 local truncation error 367, 368 timestep control 366, 367, 369 trapezoidal integration 363 .ALTER blocks 59–60 statement 60, 61, 249 AM source function 151, 151 analog transition data file 15 analysis AC 243 597 Index B accuracy 325–327 data driven 480, 481 DC 243 element template 243 Fourier 375 initialization 316 inverter 348 .MEASURE statement 243 Monte Carlo 481, 489, 489–509 optimization 515 parametric 243 POWER_ANALYSIS option 291 RC network 347, 382 statistical 484–509 Taguchi 480 temperature 480, 483 transient 243, 344 worst case 480, 484–509 yield 480 arccos(x) function 227 arcsin(x) function 227 arctan(x) function 228 arguments, command line 28, 30 arithmetic operators 227 ASCII output 28 ASIC libraries 68 asin(x) function 227 atan(x) function 228 ATEM characterization system 67 AUNIF keyword 493 autoconvergence 330 AUTOSTOP option 354 average deviation 481 average value, measuring 271 B -b argument 23 B# node name in CSOS 55 backslash continuation character 227 Backward-Euler algorithm 366 integration 366 behavioral current source 188 voltage source 176 Behavioral capacitors 83 598 Behavioral resistors 75 Biaschk 350 Bipolar Junction Transistors. See BJTs BJTs current flow 255 element template listings 300 elements, names 97 power dissipation 258 S-parameters, optimization 525 bond wire example 541 branch current output 253 breakpoint table reducing size 371 buffer 123 C C Element (capacitor) 80 capacitance element parameter 77 manufacturing variations 499 capacitor conductance requirement 334 current flow 254 element 77, 80, 296 frequency-dependent 81 linear 80 models 77 voltage controlled 189, 193 CAPOP model parameter 356 CCCS element parameter 182 CCVS element parameter 195, 196 cell characterization 480 characterization of models 323 .CHECK statements 275–281 CHGTOL option 368 circuits adder 536 description syntax 45 inverter, MOS 349 nonconvergent 338 RC network 383 reusable 63 subcircuit numbers 54 temperature 483 See also subcircuits CLOAD model parameter 204 HSPICE® Simulation and Analysis User Guide X-2005.09 Index D CMOS output driver demo 541 tristate buffer, optimization 523 command-line arguments HSPICE 22 HSPICE RF 28 commands Hspice 22–27 limit descriptors 249 output 241 comment line netlist 47 VEC files 216 common emitter gain 548 compression of input files 35 conductance for capacitors 334 pn junction 341 configuration file 14 continuation character, parameter strings 227 continuation of line netlist 47 control options accuracy 328 defaults 369 algorithm selection 324 convergence 324, 328 DC convergence 325 initialization 324 method 353 printing 249 transient analysis method 353–354 controlled sources 162, 164 CONVERGE option 329, 335 convergence control options 328 problems 335 analyzing 336 autoconverge process 330 causes 338 CONVERGE option 335 DCON setting 330 diagnosing 335–341 diagnostic tables 336 floating point overflow 335 GMINDC ramping 330 .NODESET statement 321 reducing 332 HSPICE® Simulation and Analysis User Guide X-2005.09 cos(x) function 227 cosh(x) function 228 current branch 254 controlled current sources 163, 182, 298 voltage sources 163, 195, 298 in HSPICE elements 254 output 252 sources 186 C-V plots 537 D -d argument 23 D2A function 200 input model parameters 201 model parameter 200 See also mixed mode .d2a file 200 Damped Pseudo Transient algorithm 335 data flow, overview 7 .DATA statement 56 data-driven analysis 56 data-driven analysis 480, 481 PWL source function 148 db(x) function 229 DC analysis 243, 324–325 capacitor conductances 334 initialization 324 convergence control options 324, 325 errors, reducing 332 operating point analysis 319 bypassing 345 initial conditions file 15 See also operating point sources 129 sweep 323 DC analysis measurement results file 18 DC analysis results file 18 DC initialization control options 325 .DC statement 323, 483, 515 DCCAP option 537 .DCMATCH output tables file 21 599 Index D DCON option 329, 330 DCSTEP option 334 .DCVOLT statement 321 DDL 67, 68, 548 DDLPATH environment variable 68, 548 decibel function 229 DEFAULT_INCLUDE variable 14 DEFW option 235 .DEL LIB statement 43 in .ALTER blocks 59 with .ALTER 61 with .LIB 61 with multiple .ALTER statements 60 DELAY element parameter 190, 196 delays element example 194 group 265 time (TD) 265 DELMAX option 355, 356, 370, 376 DELTA element parameter 191, 196 DELVTO model parameter 485 demo files 2n2222 BJTs transistor characterization 561 2n3330 JFETs transistor characterization 561 A/D flash converter 557 A2D 557 AC analysis 553 acl gate 554 adders 72-transistor two-bit 555 BJT NAND gate two-bit 554 BJT two-bit 553 D2A 557 MOS two-bit 554 NAND gate four-bit binary 553 air core transformer 564 algebraic output variables 552–553 parameters 552 transmission lines 568 .ALTER statement 553 AM source 567 amplifier 557 amplitude modulator 554 analog 556 AND gate 554 automatic model selection program 565 600 behavioral applications 554–555 behavioral models 556 diode 554 D-latch 554 filter 552 NAND gate 555 ring oscillator 555 triode 555 voltage to frequency converter 552 benchmarks 555–556 bisection 556 BJTs analog circuit 556 beta plot 556 differential amplifier 553, 557 diodes 556 ft plot 556 gm, gpi plots 556 photocurrent 567 Schmidt trigger 553 sense amplifier 553 BSIM3 model, LEVEL=47 564 capacitances, MOS models LEVEL=13 564 LEVEL=2 564 LEVEL=6 564 cell characterization 553, 554, 556–557 charge conservation, MOS models LEVEL=3 564 LEVEL=6 565 circuit optimization 557 CMOS differential amplifier 553 I/O driver ground bounce 553, 568 input buffer 557 inverter macro 555 output buffer 557 coax transmission line 568 crystal oscillator 553 current controlled current source 555 voltage source 555 D2A 557 DC analysis, MOS model LEVEL=34 565 DDL 557–561 delay 553, 556, 557 device optimization 561–562 differential amplifier 553 differentiator 554 HSPICE® Simulation and Analysis User Guide X-2005.09 Index D diffusion effects 553 diode photocurrent 566 D-latch 554 E Element 554 edge triggered flip-flop 554 exponential source 567 FFT AM source 562 analysis 562–563 Bartlett window 562 Blackman window 562 Blackman-Harris window 562 data-driven transient analysis 562 exponential source 562 Gaussian window 562 Hamming window 562 Hanning window 562 harmonic distortion 562 high frequency detection 562 intermodulation distortion 562 Kaiser window 563 modulated pulse source 563 Monte Carlo, Gaussian distribution 562 product of waveforms 562 pulse source 563 PWL 563 rectangular window 563 single-frequency FM source 563 sinusoidal source 562 small-signal distortion 562 switched capacitor 563 transient 562 window tests 563 filter matching 557 filters 563–564 behavioral 552 fifth-order 555, 563 fourth-order Butterworth 563 Kerwin’s circuit 563 LCR bandpass 563 matching lossy to ideal 557 ninth-order low-pass 554, 563 switched capacitor low-pass 554 FR-4 microstrip transmission line 564, 568 G Element 553, 554 GaAsFET amplifier 553 gamma model LEVEL=6 565 general applications 553–554 HSPICE® Simulation and Analysis User Guide X-2005.09 ground bounce 553, 568 group time delay 553 impact ionization plot 564 input 552 installation test 555 integrator 554 inverter 553, 554, 555, 556 characterization 556 IRF340 NMOS transistor characterization 561 I-V plots LEVEL=3 565 MOSFETS model LEVEL=13 565 SOSFETS model LEVEL=27 565 JFETs photocurrent 567 junction tunnel diode 556 LCR circuit 557 lumped MOS model 553 transmission lines 564, 568 magnetic core transformer 564 magnetics 564 microstrip transmission lines 564, 568 coupled 568 optimization 568 series 568 Monte Carlo analysis 553 Gaussian distribution 553 limit function 553 uniform distribution 553 MOS 555, 557 MOSFETs 564–565 sigma sweep 557 sweep 553 NAND gate 554, 555 NMOS E-mode model, LEVEL=8 567 noise analysis 553 op-amp 553, 554 characterization 558–560 voltage follower 555, 567 optimization 554 2n3947 Gummel model 562 DC 561 diode 561 GaAs 561 group delay 557 Hfe 561 I-V 561 JFETs 561 LEVEL=2 model beta 561 601 Index D LEVEL=28 561 MOS 561 s-parameter 561 speed, power, area 557 width 557 parameters 552 phase detector 554 locked loop 554 photocurrent 565–567 GaAs device 567 photolithographic effects 553 pll 554 pole/zero analysis 553, 563 pulse source 567 PWL 567 CCCS 555 CCVS 555 switch element 555 VCCS 554, 555 VCO 555 VCVS 555 radiation effects 565–567 bipolar devices 565–566 DC I-V, JFETs 567 GaAs differential amplifier 567 JFETs devices 566 MOSFETs devices 566 NMOS 567 RC circuit optimization 557 resistor temperature coefficients 557 RG58/AU coax test 564 ring oscillator 555 Royer magnetic core oscillator 564 Schmidt trigger 553 sense amplifier 553 series source coupled transmission lines 568 setup 556 characterization 557 shunt terminated transmission lines 568 silicon controlled rectifier 555 sine wave sampling 554, 555 single-frequency FM source 567 sinusoidal source 567 skew models 554 SNAP to HSPICE conversion 556 sources 567 s-parameters 556, 563, 565 602 sweep 553 switch 554 switched capacitor 554, 555, 567 temperature effects LEVEL=13 565 LEVEL=6 564 timing analysis 556 total radiation dose 566 transient analysis 553 transistor characterization 561 transmission lines 568 triode model 555 tunnel diodes 555, 556 twinlead transmission line model 568 U models 568 unity gain frequency 557 verilog-a 569 Viewsim A2D input 557 D2A input 557 voltage follower 555 voltage-controlled current source 554, 555 oscillator 552, 555 resistor inverter 567 voltage source 555 voltage-to-frequency converter 552 voltage-variable capacitor 554 waveform smoothing 555 worst case skew model 554 derivative, measuring 271 design name 13 Detailed Standard Parasitic Format See DSPF deviation, average 481 device characterization 67 diagnostic tables 336–337 digital files 199 vector file 208 digital output file 18 digital vector file Waveform Characteristics section 214 DIM2 parameter 266 DIM3 parameter 266 diodes breakdown example 194 HSPICE® Simulation and Analysis User Guide X-2005.09 Index E current flow 255 elements 299 equations 194 junction 96 models 95 polysilicon capacitor length 96 power dissipation 257 directories installation directory 67 TEMP 25 TMP 25 tmp 24 distortion 266 .dm# file 21 .DOUT statement 211 .dp# file 16 DSPF expansion 282, 284 selective 285 file structure 283 use requirements 284 flow, selective 285 multiple active thresholds 286 utility INE 284 DTEMP parameter 482, 483, 547 DV option 330 DVDT algorithm 363, 367 option 355, 367, 368, 369 dynamic timestep algorithm 368 E E Elements applications 163 element multiplier 178 syntax statements 171 temperature coefficients 178 time delay keyword 178 edge condition 278 electrical measurements 548 element active BJTs 97 diodes 95 JFETs 100 MESFETs 100 HSPICE® Simulation and Analysis User Guide X-2005.09 MOSFETs 102 C (capacitor) 80 IC parameter 320 identifiers 39 independent source 125, 135 L (inductor) 92 markers, mutual inductors 88 names 53 OFF parameter 318 parameters See element parameters 71 passive capacitors 77 inductor 85 mutual inductor 88 resistors 71 R (resistor) 74 statements 48, 67 current output 253 independent sources 126 Laplace 173 pole/zero 174 temperature 483 templates 267–296 analysis 243 BJTs 300 capacitor 296 current-controlled 298 function 230 independent 299 inductor 296 JFETs 302 MOSFETs 303 mutual inductor 297 resistor 296 saturable core 307 voltage-controlled 297, 298 transmission line 106, 110, 114 voltage-controlled 162 element parameters .ALTER blocks 59 BJTs 97–98 capacitors 77–79 DTEMP 482 F Elements 182–185 G Elements 186–193 H Elements 196–198 IBIS buffers 123 independent sources 126–127 603 Index F data driven PWL function 147 PULSE function 136, 139, 142, 145 SFFM function 149 inductors 86–87 JFETs and MESFETs 100–101 linear inductors 86 MOSFETs 102–104 mutual inductors, Kxxx 88 POLY 164 PWL 145, 148 resistors 72–73 transmission lines T Element 111 U Element 114 W Element 107, 107–108 .END statement for multiple HSPICE runs 61 in libraries 57 location 61 missing 36 with .ALTER 60 .ENDL statement 57 environment variables 11, 68, 548 LM_LICENSE_FILE 11 META_QUEUE 11, 12 [email protected] 12 TEMP 25 TMP 25 tmpdir 24 equations 271, 273 ERR function 272, 273 ERR1 function 273, 512 ERR2 function 273 ERR3 function 274 errors cannot open output spool file 249 DC 332 digital file has blank first line 200 file open 25 functions 272–274 internal timestep too small 319, 339, 345 missing .END statement 36 no DC path to ground 334 no input data 24 parameter name conflict 270 system resource inaccessible 249 example 604 AC analysis 262, 382 comment line 47 digital vector file 218 DSPF selective flow 285 experiments 7 HSPICE vs. SPICE methods 262 Monte Carlo 495, 502 network analysis, bipolar transistor 423 optimization 515 .OPTION (various) See individual option listings slew rate 278 transient analysis 347, 348 worst case 502 EXP source function fall time 142 initial value 142 pulsed value 142 rise time 142 exp(x) function 228 experiment 7 exponential function 142, 228 expressions, algebraic 226 external data files 44 F F Elements applications 163 multiply parameter 184 syntax statements 182 time delay keyword 185 value multiplier 184 fall time EXP source function 142 verification 276 FAST option 354 FFT analysis graph data file 18 file analog transition data 15 DC operating point initial conditions 15 initialization 14 input netlist 15 library input 15 output configuration 14 file descriptors limit 249 files .a2d 16, 200 AC analysis measurement results 17 AC analysis results 17 HSPICE® Simulation and Analysis User Guide X-2005.09 Index G .ac# 16 .d2a 200 DC analysis measurement results 18 DC analysis results 18 digital output 18 external data 44, 56 FFT analysis graph data 18, 21 .ft# 16 .gr# 16 graph data 9 hardcopy graph data 18 HBLSP analysis extraction results 18 HBLSP analysis print information 19 HBLSP analysis results 19 hspice.ini 67 .ic 16, 318 include files 43 including 14 input 9, 22 limit on number 249 .lis 17 .ls# 16, 19 .ma# 16 .ms# 16 .mt# 17 multiple simulation runs 61 names 13, ??–23 operating point node voltages 19 output listing 20 status 20 version number 22 .p2d# 16, 18 .pa# 17 .printls# 16 .printss# 16 scratch files 24, 25 .ss# 16 .ss# file 19 .st# 17 subcircuit cross-listing 21 .sw# 16 .tr# 17 transient analysis measurement results 19, 21 transient analysis results 21 files, output 16 FIND keyword 271 first character descriptions 38 HSPICE® Simulation and Analysis User Guide X-2005.09 flags, command line 28, 30 format output 292 DSPF 282, 283 NW 310 WDB 310 Fourier analysis 375 coefficients 376 equation 376 FREQ function 175 model parameter 246 frequency response table 175, 188 variable 232 frequency-dependent capacitor 81 inductor 93 FS option 370 FT option 369, 370 .ft# file 16, 18 functions A2D 200 built-in 227–231 D2A 200 DERIVATIVE 272 ERR 272 INTEG 272 LAPLACE 173, 187 NPWL 190 POLE 174, 188 PPWL 190 table 227 See also independent sources G G Elements applications 163 controlling voltages 191, 193 current 191 curve smoothing 192 element value multiplier 192 gate type 191 initial conditions 191 multiply parameter 191 names 191 605 Index H polynomial 192 resistance 191 syntax statements 186 time delay keyword 192 transconductance 192 voltage to resistance factor 192 GaAsFET model DC optimization 529 gain, calculating 262 GAUSS functions 496 keyword 493 parameter distribution 489 GEAR algorithm 363 global parameters 233 GLOBAL_LEVEL, .CHECK statement 275 GMIN option 341 GMINDC option 330, 341 GND node 54 GOAL keyword 513 .gr# file 16, 18 GRAMP option 330, 333 .GRAPH statement 242, 246, 249, 537 ground bounce checking 281 ground, node name 54 Gxxx element parameters 191 H -h argument usage information 29 H Elements applications 163 controlling voltage 198 data points 197 element multiplier 198 element name 197 gate type 197 initial conditions 197 maximum current 197 minimum current 197 syntax statements 195 time delay keyword 198 transresistance 198 H parameters 422 hardcopy graph data file 18 HBLSP analysis extraction results file 18 606 HBLSP analysis print information 19 HBLSP analysis results file 19 HD2 distortion 266 HD3 distortion 266 hertz variable 232 hierarchical designs, flattened 43 hold time verification 279 HOLD, .CHECK statement 279 HSPICE installation directory 67 starting 24 version 95.3 compatibility 369 hspice command 22–27 hspice.ini file 67 -html argument 23 hybrid (H) parameters 260 I -I argument 23 -i argument 22 IBIS buffers 123 .ic file 16, 318 IC parameter 191, 197, 320, 321 .IC statement 316, 318, 321 from .SAVE 322 .ic# file 19 ideal current sources 333 delay elements 163, 356 op-amp 163, 176, 179 transformer 163, 176, 181 IDELAY statement 214 imaginary part of AC voltage 262–263 impedance AC 266 Z parameters 260 include files 14 .INCLUDE statement 43, 60, 68, 69 independent sources AC 126, 130 AM function 151 current 126, 299 data driven PWL function 147 DC 126, 129 HSPICE® Simulation and Analysis User Guide X-2005.09 Index J elements 126 EXP function 142 functions 135 mixed types 130 PULSE function 135 PWL function 145 SFFM function 149 SIN function 139 transient 126, 130 types 135 voltage 126, 299 See also sources individual element temperature 483 inductor frequency-dependent 93 inductors current flow 254 element 85, 296 node names 86 initial conditions 317 file 15 statement 321 initialization 316, 318 file 14 saved operating point 322 initialization file 14 INOISE parameter 266 input admittance 266 analog transition data file 15 data adding library data 61 for data driven analysis 56 DC operating point initial conditions file 15 files analog transition data 15 character case 36 compression 35 DC operating point 15 demonstration 552 initialization 14 library 15 names 13, 22 netlist 15, 35 output configuration file 14 structure 43 table of components 44 impedance 266 initialization file 14 HSPICE® Simulation and Analysis User Guide X-2005.09 library file 15 netlist 45 netlist file See also input files 15, 45–61, 571 output configuration file 14 input netlist file 15 input stimuli 287 input/output cell modeling 549 installation directory $installdir 67 int(x) function 229 integer function 229 integration algorithms 363 interfaces AvanWaves 241 internal nodes, referencing 54 interstage gain 262 inverter analysis, transient 348 circuit, MOS 349 invoking HSPICE RF 28 IR drop checking 281 iterations algorithm 365 count algorithm 367 number 522 I-V and C-V plotting demo 536 J JFETs current flow 255 elements 100, 302 length 100 power dissipation 259 width 100 K keywords analysis statement syntax 515 DTEMP 482 ERR1 512 GOAL 513 LAST 271 607 Index L MONTE 490 optimization syntax 514 PAR 227 power output 257 PP 272 source functions 126 KF model parameter 386 L L Element (inductor) 92 Laplace function 173, 187 transform 173, 187 frequency 175, 188 LAST keyword 271 leadframe example 541 LENGTH model parameter 498 Levenberg-Marquardt algorithm 521 .LIB call statement 57 statement 43, 69 in .ALTER blocks 57, 59 with .DEL LIB 61 with multiple .ALTER statements 60 libraries adding with .LIB 61 ASIC cells 68 building 57 configuring 235 creating parameters 233 DDL 67 duplicated parameter names 233 .END statement 57 integrity 233 search 68 selecting 58 subcircuits 69 vendor 68 library input file 15 limit descriptors command 249 LIMIT keyword 493 line 94 line continuation VEC files 216 linear acceleration 357–?? capacitor 80 608 inductor 92 matrix reduction 357 resistor 74 .lis file 17, 20 LM_LICENSE_FILE environment variable 11 LMAX model parameter 5 LMIN model parameter 5 .LOAD statement 321 local parameters 233 truncation error algorithm 367, 368 log(x) function 228 log10(x) function 228 logarithm function 228 .ls# file 16, 19 LV 267, 268 LV18 model parameter 537 LVLTIM option 356, 367, 369 LX 268 LX7 model parameter 537 LX8 model parameter 537 LX9 model parameter 537 M M element parameter 184, 191 .ma# file 16, 17 macros 61 magnitude AC voltage 263 magnitude, AC voltage 260, 262, 263 manufacturing tolerances 497 Marquardt scaling parameter 521 MAX parameter 191, 197 max(x,y) function 229 maximum value, measuring 271 mean, statistical 481 .MEASURE statement 242, 243, 270 expression 271 failure message 269 parameters 226 measuring parameter types 269 MESFETs 100 META_QUEUE environment variable 11, 12 Meyer and Charge Conservation parameters 305 MIN parameter 191, 197 HSPICE® Simulation and Analysis User Guide X-2005.09 Index N min(x,y) function 229 minimum value, measuring 271 mixed mode See also D2A, A2D mixed sources 130 MODEL keyword 515 model parameters A2D 200 .ALTER blocks 59 capacitance distribution 499 D2A 200, 201–202 DELVTO 485 DTEMP 483 .GRAPH statement parameters 246 LENGTH 498 manufacturing tolerances 497 MONO 246 output 246 PHOTO 498 RSH 485 sigma deviations, worst case analysis 485 skew 484 TEMP 56, 483 temperature analysis 483 TIC 246 TOX 485 TREF 481, 483, 484 XPHOTO 498 model parameters See model parameters diodes .MODEL statement 483 for .GRAPH 246 models algebraic 356 characterization 323 DTEMP parameter 547 LV18 537 LX7, LX8, LX9 537 Monte Carlo analysis 489, 494, 502 reference temperature 483 specifying 68 typical set 488 MONO model parameter 246 Monte Carlo analysis 480, 481, 502–509 demo files 553 distribution options 492–493 MONTE keyword 490 MOS HSPICE® Simulation and Analysis User Guide X-2005.09 inverter circuit 349 op-amp optimization 530 MOSFETs current flow 256 drain diffusion area 102 elements 102, 303 initial conditions 103 node names 102 perimeter 103 power dissipation 259 source 103, 104 squares 103 temperature differential 103 zero-bias voltage threshold shift 104 .ms# file 16, 18 -mt argument 23 .mt# file 17, 19, 21 multiple .ALTER statements 60 multiply parameter 64, 73, 127 multipoint experiment 7 multithreading 29 mutual inductor 88, 297 N -n argument 22 NAND gate adder 536 natural log function 228 NDIM 164 .NET parameter analysis 420 netlist 43 file example 46 flat 43 input files 35 schematic 43 structure 45 netlist file example 46 network output 265, 424 nodal voltage output 252, 262 nodes connection requirements 54 floating supply 54 internal 54 MOSFET’s substrate 54 names 50, 53, 55, 537 automatic generation 55 609 Index O ground node 54 period in 51 subcircuits 53, 54 zeros in 55 numbers 50, 53 phase or magnitude difference 262 shorted 334 terminators 54 .NODESET statement 316 DC operating point initialization 321 from .SAVE 322 noise calculations 385 input 266 output 266, 386 norm of the gradient 521 NPDELAY element parameter 197 NPWL function 190 numerical integration 366 NW output format 310 O -o argument 22 ODELAY statement 214 OFF parameter 318 one-dimensional function 164 ONOISE parameter 266 .OP statement 318, 319, 345 op-amps open loops 333 optimization 530 operating point estimate 318, 345 .IC statement initialization 321 initial conditions 15 .NODESET statement initialization 321 restoring 323 saving 55, 322 solution 317, 318 transient 345 operating point information file 19 operating point node voltages file 19 operators 227 OPT keyword 514 optimization AC analysis 526 610 analysis statements 515 CMOS tristate buffer 523 control 511 convergence options 512 curve-fit 512 cv 561 data-driven vs. s-parameters 526 DC analysis 516, 519, 527, 529 example 515, 551 goal 513 incremental 527 lengths and widths 531 MODEL keyword 515 MOS 518, 530 network 520, 526 parameters 526 magnitude and phase 526 measured vs. calculated 526 results function evaluations 522 iterations 522 Marquadt scaling parameter 521 norm of the gradient 521 residual sum of squares 521 S parameters 525 simulation accuracy 512 simultaneous 523, 529, 531 statements 514 syntax 514 time analysis 513 required 511 OPTIMIZE keyword 514 .OPTION ACCT, for accounting reports 249 .ALTER blocks 59 CO, for column width 249 DCSTEP 334 INGOLD, for exponential output 249 MAXORD 373 METHOD 372 POST example 313 POST, for displaying AvanWaves plots 249 POWER_ANALYSIS 291 POWER_TOP 290 PURETP 373 SIM_ACCURACY 345, 371 SIM_ACTIVE 283, 285 HSPICE® Simulation and Analysis User Guide X-2005.09 Index O SIM_ANALOG 94 SIM_DSPF 282, 284 SIM_DSPF_ACTIVE 285 SIM_DSPF_VTOL 285 SIM_LA 283, 359 SIM_LA_FREQ 361 SIM_LA_MAXR 360 SIM_LA_MINC 360 SIM_LA_MINMODE 362 SIM_LA_TIME 361 SIM_LA_TOL 360 SIM_ORDER 373 SIM_OSC_DETECT_TOL 373 SIM_POSTAT 312 SIM_POSTDOWN 313 SIM_POSTSCOPE 313 SIM_POSTSKIP 312 SIM_POSTTOP 312 SIM_POWERPOST 290 SIM_RAIL 94 SIM_TG_THETA 373 SIM_TRAP 373 .OPTIONS POWER_ANALYSIS 291 OPTxxx parameter 512, 514 oscillators DELMAX option setting 356 output AC analysis measurement results file 17 AC analysis results file 17 admittance 266 ASCII 28 commands 241 current 253 data, redirecting 23 DC analysis measurement results file 18 DC analysis results file 18 .DCMATCH output tables file 21 digital output file 18 driver example 541 FFT analysis graph data file 18 files AC analysis measurement results 17 AC analysis results 17 DC analysis measurement results 18 DC analysis results 18 .DCMATCH output tables file 21 digital output 18 FFT analysis graph data 18 HSPICE® Simulation and Analysis User Guide X-2005.09 hardcopy data 18 HBLSP analysis extraction results 18 HBLSP analysis print information 19 HBLSP analysis results 19 names 13 operating point information 19 operating point node voltages 19 output listing 19 output status 20 redirecting 13 subcircuit cross-listing 21 transient analysis measurement results 21 transient analysis results 21 version number, specifying 22 format 292 DSPF 282 NW 310 tabulated data 309 WDB 310 graphing 246 hardcopy graph data file 18 HBLSP analysis extraction results file 18 HBLSP analysis print information 19 HBLSP analysis results file 19 impedance 266 network 265 nodal voltage, AC 262 noise 266, 386 operating point information file 19 operating point node voltages file 19 output listing file 19 output status file 20 parameters 251 power 256 .POWER statement 292 printing 249–251 redirecting 23, 28 restricting 311 reusing 287 saving 245 statements 241 subcircuit cross-listing file 21 transient analysis measurement results file 21 transient analysis results file 21 variables 243 AC formats 263 function 230 voltage 252 611 Index P output configuration file 14 output files 16 output listing file 19 output status file 20 overview of data flow 7 overview of simulation process 9 P .p2d# file 16, 18 .pa# file 17, 21 packed input files 35 PACT (linear acceleration) algorithm 358 PAR keyword 227 .PARAM statement 58, 269, 480 in .ALTER blocks 59 parameter analysis, .NET 420 parameters ACM 356 admittance (Y) 260 AF 386 algebraic 226, 227 analysis 225 assignment 224 CAPOP 356 cell geometry 232 constants 224 data type 223 data-driven analysis 56 defaults 237 defining 222, 233 DIM2 266 DIM3 266 evaluation order 223 HD2 266 HD3 266 hierarchical 64, 232, 270 hybrid (H) 260 IC 321 impedance (Z) 260 inheritance 235, 237 INOISE 266 input netlist file 42 KF 386 libraries 233–235 M 64 measurement 226 model 201, 204 612 modifying 56 multiply 226 ONOISE 266 optimization 232 OPTxxx 512, 514 output 251 overriding 234, 237 PARHIER option 237 passing 232–240 order 223 problems 240 Release 95.1 and earlier 240 repeated 270 scattering (S) 260 scope 232–233, 240 SIM2 266 simple 224 subcircuit 64 user-defined 225 UTRA 332 parametric analysis 243 PARHIER option 237 path names 54 peak-to-peak value, measuring 271 phase AC voltage 263 calculating 262 PHOTO model parameter 498 PI (linear acceleration) algorithm 359 piecewise linear sources See PWL pivot selection 354 PIVOT option 354 plot limits 245 .PLOT statement 242 simulation results 245, 249 pn junction conductance 341 POLE function 174, 188 transconductance element statement 174 voltage gain element statement 174 pole/zero conjugate pairs 174 function, Laplace transform 174, 188 POLY parameter 164, 192, 197 polynomial function 164 one-dimensional 164 three-dimensional 166 HSPICE® Simulation and Analysis User Guide X-2005.09 Index Q two-dimensional 165 [email protected] environment variable 12 POST option 9 example 313 pow(x,y) function 228 power dissipation 256, 260 function 228 output 256 stored 256 POWER keyword 257 .POWER statement 289, 294 output 292 signals 289, 290, 292 POWER_ANALYSIS option 291 POWER_TOP option 290 PP keyword 272 PPWL element parameter 192 function 190 print control options 249 .PRINT statement 242 simulation results 244, 249 printer, device specification 246 .printls# file 16, 19 .printss# file 16, 19 .PROBE statement 242, 245, 249 program structure 6 PRTDEFAULT printer 246 PULSE source function 136, 139, 142, 145 delay time 136 initial value 136 onset ramp duration 136 plateau value 136 recovery ramp duration 136 repetition period 136 width 136 PUTMEAS option 269 PWL current controlled gates 163 data driven 147 element parameter 184, 192, 197 functions 163, 167 gates 163 output values 145 parameters 145 HSPICE® Simulation and Analysis User Guide X-2005.09 repeat parameter 145 segment time values 145 simulation time 370 sources, data driven 147 voltage-controlled capacitors 163 voltage-controlled gates 163 See also data driven PWL source pwr(x,y) function 228 .PZ statement 324 Q quality assurance 480 R R Element (resistor) 74 random limit parameter distribution 490 RC analysis 347, 382 circuit 383 optimizing 520 rcells, reusing 233 real part of AC voltage 262–263 reference temperature 56, 483 RELI option 327 RELMOS option 327, 356 RELQ option 368 RELV option 327 RELVAR option 356 repeat function 535 residual sum of squares 521 resistance 381 resistor current flow 254 element 72 element template listings 296 length parameter 73 linear 74 model name 72 node to bulk capacitance 73 voltage controlled 188 width parameter 73 restricting output 311 reusing simulation output 287 rise time example 277 verify 276 613 Index S RISE, .CHECK statement 277 RLOAD model parameter 204 RMAX option 370 RMIN option 370 rms value, measuring 271 RSH model parameter 485 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 89, 307 models 87, 89 winding names 307 .SAVE statement 321 scale factors 41 SCALE parameter 72, 178, 184, 192, 198, 537 scaling, effect on delays 550 scattering (S) parameters 260 schematic netlists 43 scope of parameters 233 scratch files 24, 25 SEARCH option 69, 548 search path, setting 58 .SENS statement 324 SETUP .CHECK statement 279 time verification 279 SFFM source function carrier frequency 149 modulation index 149 output amplitude 149 output offset 149 signal frequency 149 sgn(x) function 229 shorted nodes 334 sign function 229 SIGNAME element parameter 203 signed power function 228 silicon-on-sapphire devices 55 SIM_ACCURACY option 345, 371 614 SIM_ACTIVE option 283, 285 SIM_ANALOG option 94 SIM_DELTAI options 309 SIM_DELTAV option 308 SIM_DSPF option 282, 284 SIM_DSPF_ACTIVE option 285 SIM_DSPF_SCALEC option 284 SIM_DSPF_SCALER option 284 SIM_DSPF_VTOL option 285 SIM_LA option 283, 359 SIM_LA_FREQ option 361 SIM_LA_MAXR option 360 SIM_LA_MINC option 360 SIM_LA_MINMODE option 362 SIM_LA_TIME option 361 SIM_LA_TOL option 360 SIM_POSTAT option 312, 313 SIM_POSTDOWN option 313 SIM_POSTSCOPE option 313 SIM_POSTSKIP option 312 SIM_POSTTOP option 312 SIM_POWERPOST option 290 SIM_RAIL option 94 SIM2 distortion measure 266 simulation ABSVAR option 369 accuracy 355, 512 models 356 option 357, 369 timestep 355 tolerances 325, 326, 327, 354 electrical measurements 548 example 571 graphical output 580 multiple runs 61 performance, multithreading 29 process, overview 9 reducing time 370 results graphing 246 printing 249–251 specifying 269–270 reusing output 287 speed 354 structure 6 time, RELVAR option 369 title 46 HSPICE® Simulation and Analysis User Guide X-2005.09 Index S SIN source function 139 sin(x) function 227 single point experiment 7 single-frequency FM source function 149 sinh(x) function 228 sinusoidal source function 139 skew file 488 parameters 484 slew rate example 278 verification 276 SLEW, .CHECK statement 278 SLOPETOL option simulation time 370 timestep control 369 SMOOTH element parameter 192 SONAME model parameter 204 source data driven 147 keywords 126 statements 48 See also independent sources SOVHI model parameter 204 SOVLO model parameter 204 SPICE compatibility AC output 262–263 plot 245 sqrt(x) function 228 square root function 228 .ss# file 16, 19 .st# file 17, 20 statement .CHECK 275 EDGE 278 example 276, 278, 280 HOLD 279 IR drop 281 SETUP 279 .DOUT 211 .POWER 289, 294 signals 289, 290, 292 .SURGE 274 .TRAN 289 statements .AC 483 .DATA 56 HSPICE® Simulation and Analysis User Guide X-2005.09 .DC 323, 483, 515 .DCVOLT 321 DOUT 242 element 48 .ENDL 57 .GRAPH 242, 246, 250 .IC 321 initial conditions 321 .LIB 57 .LOAD 321, 323 .MEASURE 242, 243, 268 .MODEL 483 .OP 319 .OPTION CO 249 .PARAM 58 .PLOT 242, 245, 250 .PRINT 242, 244, 250 .PROBE 242, 245, 250 .SAVE 321, 322 source 48 .STIM 242, 287 .SUBCKT 269 .TEMP 56, 483, 484 .TRAN 483 statistical analysis 484–509 statistics calculations 481 .STIM statement 242, 287 stimuli 287 structure simulation 6 subcircuit cross-listing file 21 subcircuits adder 535 calling tree 54 changing in .ALTER blocks 59 creating reusable circuits 63 hierarchical parameters 64 library structure 69 multiplying 64 node names 53, 55 output printing 249 path names 54 power dissipation computation 256 .PRINT and .PLOT statements 66 search order 66 zero prefix 55 .SUBCKT statement 269 615 Index T surge current detection 274 .SURGE statement 274 .sw# file 16, 18 sweep variables 547 switch example 193 switch-level MOSFET’s example 193 T tabular data 209 tabulated data output 309 Taguchi analysis 480 tan(x) function 227 tanh(x) function 228 TC1, TC2 element parameters 178 TD parameter 178, 185, 192, 198, 265, 271 TDELAY statement 214 TEMP directory 25 environment variable 25 model parameter 56, 483 sweep variable 547 .TEMP statement 483, 484 temper variable 232 temperature circuit 481, 483 coefficients 72, 546 derating 56, 483 element 483 optimizing coefficients 547 reference 56, 483 sweeping 547 variable 232 Temperature Variation Analysis 480 .TF statement 324 three-dimensional function 166 TIC model parameter 246 time delay 265 domain algorithm 364 variable 231 TIMESCALE model parameter 204 timestep algorithms 367 control algorithms 366–369 CHGTOL 368 616 DELMAX 370 FS 370 FT 370 minimum internal timestep 370 Minimum Timestep Coefficient 370 options 355, 369 RELQ 368 RMAX 370 RMIN 370 TRTOL 368 TSTEP 370 default control algorithm 363 DVDT algorithm 368 local truncation error algorithm 368 reversal 368 TIMESTEP model parameter 204 title for simulation 46 .TITLE statement 46 TMP directory 25 tmp directory 24 TMP environment variable 25 tmpdir environment variable 24 TNOM option 56, 483 TOX model parameter 485 .tr# file 17, 21 .TRAN statement 289, 483, 515 transconductance FREQ function 175 LAPLACE function 173 POLE function 174 transfer sign function 229 transient analysis 243 initial conditions 321, 344 inverter 348 RC network 347 sources 130 output variables 251 transient analysis measurement results file 21 transient analysis results file 21 transmission lines example 541 U Element 114 Trapezoidal (TRAP) integration algorithm 366 trapezoidal integration algorithm 363 TREF model parameter 483, 484 HSPICE® Simulation and Analysis User Guide X-2005.09 Index U triode tube 195 TRTOL option 368 truncation algorithm 367 TSTEP timestep control 370 two-dimensional function 165 U U Elements 200 digital input 199 UIC analysis parameter 318 transient analysis parameter 345 UNIF keyword 493 uniform parameter distribution 489 unity gain frequency 548 utility, INE 284 UTRA model parameter restriction 332 V -v argument version information 29 variables AC formats 263 changing in .ALTER blocks 59 DEFAULT_INCLUDE 14 Hspice-specific 231 output 243 AC 260 DC 251 transient 251 plotting 537 sweeping 547 TEMP 25 TMP 25 tmpdir 24 variables, environment 11 variance, statistical 481 VCCAP 189 VCCS See voltage controlled current source VCD format 310 VCR See voltage controlled resistor VCVS See voltage controlled voltage source vector patterns 209 vendor libraries 68 HSPICE® Simulation and Analysis User Guide X-2005.09 Verilog value format 212 version 95.3 compatibility 369 determining 29 VIH statement 215 VIL statement 215 Vnn node name in CSOS 55 VOH statement 215 VOL keyword 181 voltage failure 336 gain FREQ function 175 LAPLACE function 173 POLE function 174 initial conditions 321 logic high 215 logic low 215 nodal output DC 252 sources 171, 195, 252 summer 180 voltage-controlled capacitor 189, 193 current source 163, 182, 186, 193, 297 oscillator 181 resistor 163, 188, 193 voltage source 163, 172, 298 VREF statement 215 VTH statement 215 Vxxx source element statement 126 W W Elements 106 warnings all nodes connected together 334 floating power supply nodes 54 zero diagonal value detected 335 waveform characteristics 214 Waveform Characteristics section 214 WDB format output 310 WHEN keyword 271, 548 .WIDTH for printout width 249 wildcard uses 51 WMAX model parameter 5 617 Index X WMIN model parameter 5 worst case analysis 484, 502, 509 Worst Case Corners Analysis 480 X XGRID model parameter 246 XL model parameter 485 XMAX model parameter 247 XMIN model parameter 247 XPHOTO model parameter 498 XSCAL model parameter 247 XW model parameter 485 618 Y YGRID model parameter 246 yield analysis 480 YIN keyword 266, 424 YMAX parameter 247 YMIN parameter 247 YOUT keyword 266, 424 YSCAL model parameter 247 Z zero delay gate 181, 194 ZIN keyword 266, 424 ZOUT keyword 266, 424 HSPICE® Simulation and Analysis User Guide X-2005.09

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

Download PDF

advertisement