HSPICE® RF User Guide Version Z-2007.03, March 2007 Copyright Notice and Proprietary Information Copyright © 2007 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, Cadabra, CATS, CRITIC, CSim, Design Compiler, DesignPower, DesignWare, EPIC, Formality, HSIM, HSPICE, iN-Phase, in-Sync, Leda, MAST, ModelTools, NanoSim, OpenVera, PathMill, Photolynx, Physical Compiler, PrimeTime, SiVL, SNUG, SolvNet, System Compiler, TetraMAX, VCS, Vera, and YIELDirector are registered trademarks of Synopsys, Inc. Trademarks (™) AFGen, Apollo, Astro, Astro-Rail, Astro-Xtalk, Aurora, AvanWaves, Columbia, Columbia-CE, Cosmos, CosmosEnterprise, CosmosLE, CosmosScope, CosmosSE, DC Expert, DC Professional, DC Ultra, Design Analyzer, Design Vision, DesignerHDL, Direct Silicon Access, Discovery, Encore, Galaxy, HANEX, HDL Compiler, Hercules, Hierarchical Optimization Technology, HSIMplus, HSPICE-Link, iN-Tandem, i-Virtual Stepper, Jupiter, Jupiter-DP, JupiterXT, JupiterXT-ASIC, Liberty, Libra-Passport, Library Compiler, Magellan, Mars, Mars-Xtalk, Milkyway, ModelSource, Module Compiler, Planet, Planet-PL, Polaris, Power Compiler, Raphael, Raphael-NES, Saturn, Scirocco, Scirocco-i, Star-RCXT, Star-SimXT, Taurus, TSUPREM-4, VCS Express, VCSi, VHDL Compiler, VirSim, and VMC are trademarks of Synopsys, Inc. Service Marks (SM) MAP-in, SVP Café, and TAP-in are service marks of Synopsys, Inc. SystemC is a trademark of the Open SystemC Initiative and is used under license. ARM and AMBA are registered trademarks of ARM Limited. Saber is a registered trademark of SabreMark Limited Partnership and is used under license. All other product or company names may be trademarks of their respective owners. Printed in the U.S.A. HSPICE® RF User Guide, Z-2007.03 ii HSPICE® RF User Guide Z-2007.03 Contents 1. 2. 3. Inside This Manual. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xiii The HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xv Searching Across the HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . xvi Other Related Publications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xvi Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xvii Customer Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xviii HSPICE RF Features and Functionality . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 HSPICE RF Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1 HSPICE RF Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 HSPICE and HSPICE RF Differences . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Getting Started. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 Running HSPICE RF Simulations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 Netlist Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 Parametric Analysis Extensions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10 Generating Output Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10 HSPICE RF Output File Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11 Using the CosmosScope Waveform Display . . . . . . . . . . . . . . . . . . . . . . . . . . 12 HSPICE RF Tutorial . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15 Example 1: Using .LIN Analysis for a NMOS Low Noise Amplifier . . . . . . . . . 15 Example 2: Using HB Analysis for a Power Amplifier . . . . . . . . . . . . . . . . . . . 19 Example 3: Using HB Analysis for an Amplifier . . . . . . . . . . . . . . . . . . . . . . . . 22 Device Model Cards . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27 Example 4: Using HBOSC Analysis for a Colpitts Oscillator . . . . . . . . . . . . . . 28 Example 5: Using HBOSC Analysis for a CMOS GPS VCO . . . . . . . . . . . . . . 31 Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer . . . . . . . . . 38 iii Contents Two-tone HB Approach . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 HBAC Approach . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Comparing Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41 Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 4. iv Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 Shooting Newton Analysis Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43 Driven Phase Frequency Example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Ring Oscillator Example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 Other Shooting Newton Analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54 Demonstration Input Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Input Netlist and Data Entry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 Input Netlist File Guidelines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 57 Input Line Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58 Delimiters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 Node Identifiers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 Instance Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 Hierarchy Paths . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66 Numbers. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66 Parameters and Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67 Input Netlist File Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68 Schematic Netlists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68 Input Netlist File Composition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70 Title of Simulation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 Comments and Line Continuation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 Element and Source Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 72 Defining Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 Node Naming Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75 Element, Instance, and Subcircuit Naming Conventions . . . . . . . . . . . . . 78 Subcircuit Node Names . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78 Path Names of Subcircuit Nodes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 79 Automatic Node Name Generation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 80 Global Node Names. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 80 Circuit Temperature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 80 Data-Driven Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81 Library Calls and Definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81 Contents Defining Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5. 6. 82 Deleting a Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85 Ending a Netlist . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86 Condition-Controlled Netlists (IF-ELSE). . . . . . . . . . . . . . . . . . . . . . . . . . 86 Using Subcircuits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87 Hierarchical Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88 DDL Library Access . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91 Vendor Libraries. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92 Subcircuit Library Structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93 Parameters and Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Using Parameters in Simulation (.PARAM) . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Defining Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Assigning Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97 User-Defined Function Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 98 Predefined Analysis Function. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Measurement Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 .PRINT and .PROBE Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Using Algebraic Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Built-In Functions and Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100 Parameter Scoping and Passing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104 Library Integrity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105 Reusing Cells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106 Creating Parameters in a Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106 Parameter Defaults and Inheritance. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108 Parameter Passing Solutions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111 Testbench Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 Passive Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 Resistors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 114 Capacitors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119 Inductors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125 Multi-Terminal Linear Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 W-element (Distributed Transmission Lines) . . . . . . . . . . . . . . . . . . . . . . 139 T-element (Ideal Transmission Lines). . . . . . . . . . . . . . . . . . . . . . . . . . . . 143 v Contents 7. vi Scattering Parameter Data Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . 147 Port Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Port Element Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Using the Port Element for Mixed-Mode Measurement . . . . . . . . . . . . . . 159 Active Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 Diode Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 Bipolar Junction Transistor (BJT) Element . . . . . . . . . . . . . . . . . . . . . . . . 162 JFETs and MESFETs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164 MOSFETs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166 Steady-State Voltage and Current Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . 169 I and V Element Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 169 Steady-State HB Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 172 Phase Differences Between HB and SIN Sources . . . . . . . . . . . . . . . . . . . . . 174 Behavioral Noise Sources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 175 Power Supply Current and Voltage Noise Sources . . . . . . . . . . . . . . . . . 176 Function Approximations for Distributed Devices . . . . . . . . . . . . . . . . . . . . . . 178 Foster Pole-Residue Form for Transconductance or Gain . . . . . . . . . . . . 178 Advantages of Foster Form Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . 178 G and E Element Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 179 Complex Signal Sources and Stimuli . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 180 Vector-Modulated RF Source. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 180 Voltage and Current Source Elements. . . . . . . . . . . . . . . . . . . . . . . . . . . 182 SWEEPBLOCK in Sweep Analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 189 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 190 Using SWEEPBLOCK in a DC Parameter Sweep . . . . . . . . . . . . . . . . . . 190 Using in Parameter Sweeps in TRAN, AC, and HB Analyses . . . . . . . . . 191 Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 191 Clock Source with Random Jitter. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 191 Syntax of SIN, COS, and Pulse Sources . . . . . . . . . . . . . . . . . . . . . . . . . 192 References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 195 Steady-State Harmonic Balance Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . 197 Harmonic Balance Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 198 Harmonic Balance Equations. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199 Features Supported . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 200 Contents Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8. 9. 200 HB Analysis Spectrum . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 201 HB Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 203 Harmonic Balance Output Measurements . . . . . . . . . . . . . . . . . . . . . . . . 205 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 206 Calculating Power Measurements After HB Analyses . . . . . . . . . . . . . . . 208 Calculations for Time-Domain Output . . . . . . . . . . . . . . . . . . . . . . . . . . . 211 Output Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 212 Using .MEASURE with .HB Analyses . . . . . . . . . . . . . . . . . . . . . . . . . . . 212 HB Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 214 Errors and Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 216 References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 218 Steady-State Shooting Newton Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . 219 SN Steady-State Time Domain Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 219 SN Analysis Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 220 SN Analysis Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 222 Shooting Newton with Fourier Transform (.SNFT) . . . . . . . . . . . . . . . . . . . . . . 224 .SNFT Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 225 Oscillator and Phase Noise Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 229 Harmonic Balance or Shooting Newton for Oscillator Analysis . . . . . . . . . . . . 229 Harmonic Balance Analysis for Frequency of Oscillation. . . . . . . . . . . . . . . . . 229 Input Syntax for Harmonic Balance Oscillator Analysis . . . . . . . . . . . . . . . . . . 230 HB Simulation of Ring Oscillators . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233 HBOSC Analysis Using Transient Initialization . . . . . . . . . . . . . . . . . . . . . . . . 234 Additional .HBOSC Analysis Options. . . . . . . . . . . . . . . . . . . . . . . . . . . . 235 .HBOSC Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 236 Oscillator Analysis Using Shooting Newton (.SNOSC) . . . . . . . . . . . . . . . . . . 236 Phase Noise Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 238 PHASENOISE Input Syntax. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 240 Phase Noise Algorithms. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 242 Measuring PHASENOISE Analyses with .MEASURE . . . . . . . . . . . . . . . 243 PHASENOISE Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 245 vii Contents Phase Noise Analysis Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . viii 248 Jitter Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 248 Jitter Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 251 .MEASURE Statements to Support Jitter Analysis . . . . . . . . . . . . . . . . . 251 RMS JITTER Measurement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 255 References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 256 10. Large Signal Periodic AC, Transfer Function, and Noise Analyses . . . . . 257 Multitone Harmonic Balance AC Analysis (.HBAC) . . . . . . . . . . . . . . . . . . . . . 257 Prerequisites and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 258 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 258 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 259 HBAC Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 261 Errors and Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 262 Shooting Newton AC Analysis (.SNAC) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 263 Prerequisites and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 263 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 264 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 264 SNAC Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 266 Errors and Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 267 SNAC Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 267 Multitone Harmonic Balance Noise (.HBNOISE) . . . . . . . . . . . . . . . . . . . . . . . 268 Supported Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271 Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 272 Measuring HBNOISE Analyses with .MEASURE . . . . . . . . . . . . . . . . . . 273 Errors and Warnings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274 HBNOISE Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274 Shooting Newton Noise Analysis (.SNNOISE) . . . . . . . . . . . . . . . . . . . . . . . . 275 Supported Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 275 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 276 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 278 Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 279 Measuring SNNOISE Analyses with .MEASURE . . . . . . . . . . . . . . . . . . 279 SNNOISE Analysis Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 280 Contents Periodic Time-Dependent Noise Analysis (.PTDNOISE) . . . . . . . . . . . . . . . . . 281 PTDNOISE Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 282 PTDNOISE Output Syntax and File Format. . . . . . . . . . . . . . . . . . . . . . . 284 Error Handling and Warnings. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 287 Multitone Harmonic Balance Transfer Function Analysis (.HBXF). . . . . . . . . . 287 Supported Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 288 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 289 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 289 Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 290 Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 290 HBXF Test Listing. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 291 Shooting Newton Transfer Function Analysis (.SNXF). . . . . . . . . . . . . . . . . . . 291 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 291 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 292 Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 293 Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 293 SNXF Test Listing. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 294 References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 295 11. S-parameter Extraction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 297 Frequency Translation S-Parameter (HBLIN) Extraction . . . . . . . . . . . . . . . . . 298 HB Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 300 Port-element. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301 HBLIN Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 301 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 304 Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 305 Large-Signal S-parameter (HBLSP) Analysis . . . . . . . . . . . . . . . . . . . . . . . . . 305 Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 306 Input Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 309 Output Data Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 309 12. Envelope Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 Envelope Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 311 Envelope Analysis Commands. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 312 Output Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 315 ix Contents x Envelope Output Data File Format. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 315 13. Post-Layout Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317 Post-Layout Back-Annotation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 317 Standard Post-Layout Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 319 Selective Post-Layout Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 322 Additional Post-Layout Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 324 Selective Extraction Flow . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 326 Overview of DSPF Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 327 Overview of SPEF Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 333 Linear Acceleration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 344 PACT Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 346 PI Algorithm . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 346 Linear Acceleration Control Options Summary . . . . . . . . . . . . . . . . . . . . 347 14. Statistical and Monte Carlo Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 349 Overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 349 Application of Statistical Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 349 Analytical Model Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 350 Simulating Circuit and Model Temperatures . . . . . . . . . . . . . . . . . . . . . . . . . . 351 Temperature Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 352 .TEMP Statement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Worst Case Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Model Skew Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 354 Monte Carlo Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 359 Monte Carlo Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 360 Monte Carlo Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 362 .PARAM Distribution Function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 362 Monte Carlo Parameter Distribution . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 364 Monte Carlo Examples. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 365 Worst Case and Monte Carlo Sweep Example . . . . . . . . . . . . . . . . . . . . . . . . 371 Transient Sigma Sweep Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 373 Monte Carlo Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 374 Simulating the Effects of Global and Local Variations with Monte Carlo . . . . . 381 Variations Specified on Geometrical Instance Parameters . . . . . . . . . . . 381 Contents Variations Specified in the Context of Subcircuits . . . . . . . . . . . . . . . . . . 382 Variations on a Model Parameter Using a Local Model in Subcircuit. . . . 384 Indirect Variations on a Model Parameter . . . . . . . . . . . . . . . . . . . . . . . . 384 Variations Specified on Model Parameters . . . . . . . . . . . . . . . . . . . . . . . 385 Variations Specified Using DEV and LOT . . . . . . . . . . . . . . . . . . . . . . . . 386 Combinations of Variation Specifications . . . . . . . . . . . . . . . . . . . . . . . . . 386 15. Using HSPICE with HSPICE RF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 389 RF Numerical Integration Algorithm Control . . . . . . . . . . . . . . . . . . . . . . . . . . 389 RF Transient Analysis Accuracy Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 389 .OPTION SIM_ACCURACY . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 390 Algorithm Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 390 RF Transient Analysis Output File Formats . . . . . . . . . . . . . . . . . . . . . . . . . . . 392 Tabulated Data Output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 393 WDB Output Format. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 393 TR Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 394 XP Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 394 NW Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 394 VCD Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 394 turboWave Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 Undertow Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 CSDF Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 395 Compressing Analog Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 396 Eliminating Voltage Datapoints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 396 Eliminating Current Datapoints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 396 16. Advanced Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 399 Creating a Configuration File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 399 Inserting Comments in a .hspice File. . . . . . . . . . . . . . . . . . . . . . . . . . . . 402 Using Wildcards in HSPICE RF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 402 Limiting Output Data Size . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 403 SIM_POSTTOP Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 403 SIM_POSTSKIP Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 SIM_POSTAT Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 SIM_POSTDOWN Option . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 404 SIM_POSTSCOPE Option. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 405 xi Contents xii Probing Subcircuit Currents . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 405 Generating Measurement Output Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 407 Optimization . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 407 Optimizing AC, DC. and TRAN Analyses . . . . . . . . . . . . . . . . . . . . . . . . . 409 Optimizing HB Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 409 Optimizing HBOSC Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 410 Using CHECK Statements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 411 Setting Global Hi/Lo Levels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 412 Slew, Rise, and Fall Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 412 Edge Timing Verification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 413 Setup and Hold Verification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 414 IR Drop Detection. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 415 POWER DC Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 415 Power DC Analysis Output Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 416 POWER Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 417 Setting Default Start and Stop Times. . . . . . . . . . . . . . . . . . . . . . . . . . . . 418 Controlling Power Analysis Waveform Dumps . . . . . . . . . . . . . . . . . . . . . 418 Detecting and Reporting Surge Currents. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 418 Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 421 About This Guide This manual contains detailed reference information, application examples, and design flow descriptions that show how HSPICE RF features can be used for RF circuit characterization. The manual supplements the HSPICE user documentation by describing the additional features, built on top of the standard HSPICE feature set, that support the design of RF and high-speed circuits. Where necessary, the manual describes differences that might exist between HSPICE RF and HSPICE. Note: This manual discusses only HSPICE RF features. For information on other HSPICE applications, see the other HSPICE manuals, listed in The HSPICE Documentation Set on page xv. Inside This Manual This manual contains the chapters described below. For access to the other manuals in the HSPICE documentation set, see the next section, Searching Across the HSPICE Documentation Set on page xvi. Chapter Description Chapter 1, HSPICE RF Features and Functionality Introduces HSPICE RF features and functionality. Chapter 2, Getting Started Describes how to set up your environment, invoke HSPICE RF, customize your simulation, and redirect input and output. Chapter 3, HSPICE RF Tutorial Provides a quick-start tutorial for users new to HSPICE RF. Chapter 4, Input Netlist and Data Entry Describes the input netlist file and methods of entering data in HSPICE or HSPICE RF. Chapter 5, Parameters and Functions Describes how to use parameters within HSPICE RF netlists. HSPICE® RF User Guide Z-2007.03 xiii About This Guide Inside This Manual xiv Chapter Description Chapter 6, Testbench Elements Describes the specialized elements supported by HSPICE RF for high-frequency analysis and characterization and the syntax for the basic elements of a circuit netlist in HSPICE or HSPICE RF. Chapter 7, Steady-State Harmonic Balance Analysis Describes how to use harmonic balance analysis for frequency-driven, steady-state analysis. Chapter 8, Steady-State Shooting Newton Analysis Describes HSPICE RF steady-state time domain analysis based on Shooting-Newton. Chapter 9, Oscillator and Phase Noise Analysis Describes how to use HSPICE RF to perform oscillator and phase noise analysis on autonomous (oscillator) circuits. Chapter 10, Large Signal Periodic AC, Transfer Function, and Noise Analyses Describes how to use harmonic balance-based and Shooting Newton AC analysis as well as nonlinear, steady-state noise analysis and XF analysis. Chapter 11, S-parameter Extraction Describes how to use periodically driven nonlinear circuit analyses as well as noise parameter calculation. Chapter 12, Envelope Analysis Describes how to use envelope simulation. Chapter 13, Post-Layout Analysis Describes the post-layout flow, including postlayout back-annotation, DSPF and SPEF files, linear acceleration, check statements, and power analysis. Chapter 14, Statistical and Monte Carlo Analysis Describes the features available in HSPICE RF for statistical analysis. Chapter 15, Using HSPICE with HSPICE RF Describes how various analysis features differ in HSPICE RF as compared to standard HSPICE. Chapter 16, Advanced Features Describes how to invoke HSPICE RF and how to perform advanced tasks, including redirecting input and output. HSPICE® RF User Guide Z-2007.03 About This Guide 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® RF User Guide Provides reference information for HSPICE and HSPICE RF commands and options. HSPICE 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. HSPICE MOSFET Models Manual Describes standard MOSFET models you can use when simulating your circuit designs in HSPICE. HSPICE RF User Guide Describes a special set of analysis and design capabilities added to HSPICE to support RF and highspeed circuit design. AMS Discovery Simulation Interface Guide for HSPICE Describes use of the Simulation Interface with other EDA tools for HSPICE. AvanWaves User Guide Describes the AvanWaves tool, which you can use to display waveforms generated during HSPICE circuit design simulation. HSPICE® RF User Guide Z-2007.03 xv About This Guide Searching Across the HSPICE Documentation Set Searching Across the HSPICE Documentation Set You can access the PDF format documentation from your install directory for the current release by entering -docs on the terminal command line when the HSPICE tool is open. Synopsys includes an index with your HSPICE documentation that lets you search the entire HSPICE documentation set for a particular topic or keyword. In a single operation, you can instantly generate a list of hits that are hyperlinked to the occurrences of your search term. For information on how to perform searches across multiple PDF documents, see the HSPICE release notes (available on SolvNet at http://solvnet.synopsys.com/ReleaseNotes) or the Adobe Reader online help. Note: To use this feature, the HSPICE documentation files, the Index directory, and the index.pdx file must reside in the same directory. (This is the default installation for Synopsys documentation.) Also, Adobe Acrobat must be invoked as a standalone application rather than as a plug-in to your web browser. You can also invoke HSPICE and RF documentation in a browser-based help system by entering-help on your terminal command line when the HSPICE tool is open. This provides access to all the HSPICE manuals with the expection of the AvanWaves User Guide which is available in PDF format only. Other Related Publications For additional information about <Product Name>, see: ■ The HSPICE release notes, available on SolvNet (see Known Limitations and Resolved STARs, below) ■ Documentation on the Web, which provides PDF documents and is available through SolvNet at http://solvnet.synopsys.com/DocsOnWeb You might also want to refer to the documentation for the following related Synopsys products: xvi ■ CosmosScope ■ Aurora HSPICE® RF User Guide Z-2007.03 About This Guide Conventions ■ Raphael ■ VCS Known Limitations and Resolved STARs You can find information about known problems and limitations and resolved Synopsys Technical Action Requests (STARs) in the <Product Name> Release Notes in SolvNet. To see the latest <Product Name> Release Notes: 1. Go to https://solvnet.synopsys.com/ReleaseNotes. (If prompted, enter your user name and password. If you do not have a Synopsys user name and password, follow the instructions to register with SolvNet.) 2. Click <Product Name>, then click the release you want in the list that appears at the bottom. Conventions The following conventions are used in Synopsys documentation. Convention Description Courier Indicates command syntax. Italic Indicates a user-defined value, such as object_name. Bold Indicates user input—text you type verbatim—in syntax and examples. [ ] Denotes optional parameters, such as: write_file [-f filename] ... Indicates that parameters can be repeated as many times as necessary: pin1 pin2 ... pinN | Indicates a choice among alternatives, such as low | medium | high \ HSPICE® RF User Guide Z-2007.03 Indicates a continuation of a command line. xvii About This Guide Customer Support Convention Description / Indicates levels of directory structure. Edit > Copy Indicates a path to a menu command, such as opening the Edit menu and choosing Copy. Control-c Indicates a keyboard combination, such as holding down the Control key and pressing c. Customer Support Customer support is available through SolvNet online customer support and through contacting the Synopsys Technical Support Center. Accessing SolvNet SolvNet includes an electronic knowledge base of technical articles and answers to frequently asked questions about Synopsys tools. SolvNet also gives you access to a wide range of Synopsys online services, which include downloading software, viewing Documentation on the Web, and entering a call to the Support Center. To access SolvNet: 1. Go to the SolvNet Web page at http://solvnet.synopsys.com. 2. If prompted, enter your user name and password. (If you do not have a Synopsys user name and password, follow the instructions to register with SolvNet.) If you need help using SolvNet, click Help on the SolvNet menu bar. xviii HSPICE® RF User Guide Z-2007.03 About This Guide Customer Support Contacting the Synopsys Technical Support Center If you have problems, questions, or suggestions, you can contact the Synopsys Technical Support Center in the following ways: ■ Open a call to your local support center from the Web by going to http://solvnet.synopsys.com/EnterACall (Synopsys user name and password required). ■ Send an e-mail message to your local support center. ■ • E-mail [email protected] from within North America. • Find other local support center e-mail addresses at http://www.synopsys.com/support/support_ctr. Telephone your local support center. • Call (800) 245-8005 from within the continental United States. • Call (650) 584-4200 from Canada. • Find other local support center telephone numbers at http://www.synopsys.com/support/support_ctr. HSPICE® RF User Guide Z-2007.03 xix About This Guide Customer Support xx HSPICE® RF User Guide Z-2007.03 1 HSPICE RF Features and Functionality 1 Introduces HSPICE RF features and functionality. HSPICE RF is a special set of analysis and design capabilities that support the design of RF and high-speed circuits. This functionality, built on top of the standard HSPICE feature set, is also useful for analog and signal integrity applications. Although the HSPICE and HSPICE RF simulators share a common set of device models and simulation capabilities, HSPICE RF includes several modeling, simulation, and measurement additions that augment the ultimate-accuracy analog circuit simulation capabilities of HSPICE. Note: This manual describes the additional features and capabilities of HSPICE RF. Where necessary, the manual describes differences between HSPICE RF and HSPICE. For information about standard HSPICE device models, syntax, and simulation control, you can refer to one of the other HSPICE manuals in the HSPICE documentation set, listed in The HSPICE Documentation Set on page xv. HSPICE RF Overview HSPICE RF consists of: ■ The hspicerf simulation engine ■ The CosmosScope (cscope) waveform display tool The hspicerf simulation engine contains extensions to HSPICE for RF design. These extensions are in the form of new analysis commands and new elements. The hspicerf simulation engine processes command and element syntax for new RF simulation features but also accepts standard HSPICE netlist files as input. HSPICE® RF User Guide Z-2007.03 1 Chapter 1: HSPICE RF Features and Functionality HSPICE RF Overview The CosmosScope waveform display tool has been enhanced with special features for reading and analyzing data created by the HSPICE RF simulation engine. For a basic overview on how to use CosmosScope to view HSPICE RF output, see Using the CosmosScope Waveform Display on page 12. HSPICE RF Features This section briefly introduces the features of both the simulation engine and the waveform display tool. HSPICE RF supports most HSPICE capabilities, and also includes: ■ Steady-state frequency-domain analyses for linear and nonlinear circuits. ■ High-performance transient analysis for faster simulation of high-speed digital and analog circuits. ■ Port-wise automated .AC analyses for S (scattering) parameters. The.LIN command invokes extraction of noise and linear transfer parameters of a multi-port linear network. Extracts the S parameter and generates the Nport model. This command is used in conjunction with the .AC command to measure multiport S, Y, and Z parameters, noise parameters, stability and gain factors, and matching coefficients. Additionally, it is used with the Port element, which identifies the network ports and their impedances. You can also use mixed mode with .LIN. 2 ■ The Port (P) element identifies ports used in LIN analysis (multiport S, Y, or Z parameter and noise parameter extraction). A port element behaves as a noiseless impedance or a voltage source in series with an impedance, depending on the simulation being performed. Different impedances can be specified for DC, transient, AC, HB, and HBAC analyses. ■ The S element describes a linear network using multi-port S, Y, or Z parameters in the form of a frequency table. These parameters can come from a .LIN simulation or from physical measurement. The standard Touchstone and CITIfile formats are supported in addition to a proprietary HSPICE format. ■ The syntax of voltage and current sources as well as Port elements supports the syntax for specifying power sources. In this case, the source value is interpreted as a power value in Watts or dBm units, and the Port element is HSPICE® RF User Guide Z-2007.03 Chapter 1: HSPICE RF Features and Functionality HSPICE RF Overview implemented as a voltage source with a series impedance. The.HBLSP command invokes periodically driven nonlinear circuit analyses for powerdependent S parameters. ■ Harmonic Balance (.HB) analysis using Direct and Krylov solvers. The.HB command invokes the single and multitone Harmonic Balance algorithm for periodic steady state analysis. ■ TRANFORHB element parameter to recognize V/I sources that include SIN and PULSE transient descriptions as well as PWL and VMRF sources. ■ Harmonic balance-based periodic AC analysis. The .HBAC command invokes periodic AC analysis for analyzing small-signal perturbations on circuits operating in a large-signal periodic steady state. ■ Harmonic Balance-based Periodic Noise analysis (.HBNOISE) for noise analysis of periodically modulated circuits, includes stationary, cyclostationary, and frequency-dependent noise effects. ■ Autonomous Harmonic Balance analysis. The.HBOSC command invokes the multitone, oscillator-capable Harmonic Balance algorithm for periodic steady state analysis. ■ Perturbation analysis for Oscillator Phase Noise. The .HBAC command invokes phase periodic AC noise for oscillators circuits operating in a largesignal steady-state. ■ Oscillator phase noise analysis, including both a nonlinear perturbation method and a PAC method, and includes stationary, cyclostationary, frequency-dependent, and correlated noise effects. ■ Frequency translation S-parameter and noise figure extraction with the .HBLIN command. ■ Envelope analysis. The.ENV command: invokes standard envelope simulation. The .ENVOSC command invokes envelope startup simulation. The.ENVFFT command invokes envelope Fast Fourier Transform simulation. ■ .OPTION HBTRANINIT, HBTRANPTS, and HBTRANSTEP for transient analysis of ring oscillators. ■ Convolution for transient analysis of S parameter data models (S-element). ■ Calculation of the transfer function from an arbitrary source and harmonic in the circuit to a designated output with the .HBXF command. ■ Reading encrypted netlists. HSPICE® RF User Guide Z-2007.03 3 Chapter 1: HSPICE RF Features and Functionality HSPICE RF Overview ■ .OPTION SIM_ACCURACY provides simplified accuracy control for all simulations while .OPTION SIM_ORDER and SIM_TRAP improve transient analysis simulation controls. ■ DSPF Flow for fast analysis using parasitic data from layout. ■ .OPTION SIM_LA provides linear acceleration for RC network reduction for faster simulation. ■ Saving .PRINT simulation output to a separate file. ■ HERTZ variable for frequency-dependent equations. ■ IC=OFF in element statements, IC parameter (initial conditions). ■ Shooting Newton steady-state time domain analysis; the Shooting Newton algorithm provides functionality to support the following commands: .SN, .SNAC .SNFT, .SNNOISE, .SNOSC, and .SNXF. ■ Periodic Time-Dependent Noise Analysis (.PTDNOISE) calculates the noise spectrum and the total noise at a point in time. Jitter in a digital threshold circuit can then be determined from the total noise and the digital signal slew rate. HSPICE RF also adds the following measurement capabilities to HSPICE: ■ Small-signal scattering parameters. ■ Small-signal two-port noise parameters. ■ 1 dB compression point. ■ Intercept points (for example, IP2, IP3). ■ Mixer conversion gain and noise figure. ■ VCO output spectrum. ■ Oscillator phase noise. Options simplify specifying levels of accuracy. As a result, HSPICE RF provides effective simulation solutions for RF, high-speed, and PCB signal integrity circuit challenges. 4 HSPICE® RF User Guide Z-2007.03 Chapter 1: HSPICE RF Features and Functionality HSPICE and HSPICE RF Differences HSPICE and HSPICE RF Differences The following tables give an overview of which features (Table 1) and device models (Table 2 on page 7) in HSPICE are not supported in HSPICE RF. Table 1 HSPICE Features Not in HSPICE RF Feature See Read hspice.ini file. HSPICE Simulation and Analysis User Guide Short names for internal sub-circuits, such as 10:M1. HSPICE Simulation and Analysis User Guide .MODEL types: AMP and PLOT for graphs HSPICE and RF Command Reference Parameter definition (.PARAM) for Monte Carlo statistical functions HSPICE and RF Command Reference .PLOT simulation output HSPICE and RF Command Reference .GRAPH simulation output (uses PLOT model type) HSPICE Simulation and Analysis User Guide HSPICE and RF Command Reference .WIDTH, and .OPTION CO HSPICE Simulation and Analysis User Guide HSPICE and RF Command Reference .OPTION ACCT HSPICE Simulation and Analysis User Guide HSPICE and RF Command Reference Element template output HSPICE Simulation and Analysis User Guide Group time delay parameters in AC analysis output HSPICE Simulation and Analysis User Guide .DISTO distortion analysis and associated output commands HSPICE Simulation and Analysis User Guide .SAVE and .LOAD HSPICE and RF Command Reference HSPICE® RF User Guide Z-2007.03 5 Chapter 1: HSPICE RF Features and Functionality HSPICE and HSPICE RF Differences Table 1 HSPICE Features Not in HSPICE RF (Continued) Feature See Options that activate unsupported features in HSPICE RF: FAST GSHDC GSHUNT LIMPTS OFF RESMIN TIMERES All version options HSPICE and HSPICE RF Command Reference Options ignored by HSPICE RF, because they are not needed since they are replaced by automated algorithms: ABSH ABSV ABSVAR BELV BKPSIZ CHGTOL CONVERGE CSHDC CVTOL DCFOR DCHOLD DCON DCSTEP DI DV DVDT FAST FS FT GMAX GRAMP GSHDC GSHUNT ICSWEEP IMAX IMIN ITL3 ITL5 ITLPZ LIMPTS LVLTIM MAXAMP MBYPASS NEWTOL RELH RELI RELQ RELV RELVAR TRTOL All matrix options All error options HSPICE and HSPICE RF Command Reference Some Transient/AC input/output (I/O) options. HSPICE RF does support POST and PROBE options. Sub-circuit cross-listing in a .pa file HSPICE Simulation and Analysis User Guide, Chapter 3 -r command-line argument for a remote host HSPICE Simulation and Analysis User Guide .OP supports node voltage for any time, but supports element values only for t=0. HSPICE and HSPICE RF Command Reference Sensitivity analysis (.SENS) HSPICE Simulation and Analysis User Guide HSPICE and HSPICE RF Command Reference 6 HSPICE® RF User Guide Z-2007.03 Chapter 1: HSPICE RF Features and Functionality HSPICE and HSPICE RF Differences Table 1 HSPICE Features Not in HSPICE RF (Continued) Feature See DC mismatch analysis (.DCMATCH) HSPICE Simulation and Analysis User Guide HSPICE and HSPICE RF Command Reference Table 2 Device Models Not in HSPICE RF Model See B element: IBIS buffer— HSPICE Signal Integrity Guide Bname n1 n2 [...] parameters data-driven I element (current source) HSPICE Elements and Device Models Manual data-driven V element (voltage source) HSPICE Elements and Device Models Manual BJT LEVEL=10 (MODELLA) HSPICE Elements and Device Models Manual, Chapter 5 MOSFET Levels 4-8. HSPICE MOSFET Models Manual Common Model Interface (CMI) HSPICE MOSFET Models Manual HSPICE® RF User Guide Z-2007.03 7 Chapter 1: HSPICE RF Features and Functionality HSPICE and HSPICE RF Differences 8 HSPICE® RF User Guide Z-2007.03 2 Getting Started 2 Describes how to set up your environment, invoke HSPICE RF, customize your simulation, redirect input and output, and use the CosmosScope waveform display tool. Before you run HSPICE RF, you need to set up several environment variables. You can also create a configuration file to customize your simulation run. HSPICE RF accepts a netlist file from standard input and delivers the ASCII text simulation results to HTML or to standard output. Error and warning messages are forwarded to standard error output. Running HSPICE RF Simulations Use the following syntax to invoke HSPICE RF: hspicerf [-a] inputfile [outputfile] [-h] [-v] For a description of the hspicerf command syntax and arguments, see section HSPICE RF Command Syntax in the HSPICE and HSPICE RF Command Reference. Netlist Overview The circuit description syntax for HSPICE RF is compatible with the SPICE and HSPICE input netlist format. For a description of an input netlist file and methods of entering data, see chapter Input Netlist and Data Entry in the HSPICE Simulation and Analysis User Guide. HSPICE® RF User Guide Z-2007.03 9 Chapter 2: Getting Started Parametric Analysis Extensions Parametric Analysis Extensions All major HSPICE RF analyses (.TRAN, .AC, .DC, and .HB) support the following parameter sweeps with the same syntax as standard HSPICE: ■ LIN ■ DEC ■ OCT ■ DATA ■ POI You can also use the MONTE keyword for a Monte Carlo analysis or the OPTIMIZE keyword for optimization. Generating Output Files HSPICE RF generates a table of simulation outputs. ■ If the output is text (the default), the text is put into a .lis file. ■ If you specify .OPTION POST, then HSPICE RF generates simulation output in a format suitable for a waveform display tool. ■ The default output format for transient analysis in HSPICE RF is the same as in HSPICE: the .tr0 file format. For additional information, see Standard Output Files in the HSPICE Simulation and Analysis User Guide. The Synopsys interactive waveform display tool, CosmosScope, can display both the text simulation results and binary output within the X-window environment. All output functions (.PRINT, .PROBE, .MEASURE, and so on) can use power output variables in the form p(devicename), just as in HSPICE. You can also use the “power” keyword. Larger output files from multi-million transistor simulations might not be readable by some waveform viewers. Options are available that enable you to limit the output file size. See Limiting Output Data Size on page 403 for more information. 10 HSPICE® RF User Guide Z-2007.03 Chapter 2: Getting Started Generating Output Files HSPICE RF Output File Types Table 3 shows the output file extensions that HSPICE RF analyses produce. The base file name of each output file is the same as the input netlist file’s base name. The # at the end of each file extension represents the .ALTER run from which the file came. In general, text output from .PRINT commands is intended to be read by humans, while binary output from .PROBE or .OPTION POST is intended to be read by the CosmosScope waveform display tool. Table 3 HSPICE RF Output File Types Command Text Output Output for CosmosScope AC analysis (.AC) .printac# .ac# AC noise analysis (.NOISE) .printac# .ac# DC sweep (.DC) .printsw# .sw# Envelope analysis (.ENV) .printev# .ev# Envelope FFT (.ENVFFT) (none) .fe# Harmonic Balance (.HB) .printhb# .hb# Harmonic Balance AC (.HBAC) .printhb# .hb# .HBLIN analysis .PRINT output: .printhl# S-param output: .SnP .PROBE output: .hl# S-paramr output: .SnP .HBLSP large-signal .PRINT output: .printls# S-param output: .p2d# .PROBE output: .ls# S-param output: .p2d# .HBLSP small-signal .PRINT output: .printss# S/noise output: .S2P# .PROBE output: .ss# S/noise output: .S2P# HBAC noise (.HBNOISE) .printsnpn# .pn# Harmonic Balance OSC (.HBOSC) .printhb# .hb# HSPICE® RF User Guide Z-2007.03 11 Chapter 2: Getting Started Using the CosmosScope Waveform Display Table 3 HSPICE RF Output File Types Command Text Output Output for CosmosScope Harmonic Balance TRAN (.HBTRAN) .printhr# .hr# Transfer Functions (.HBXF) .printxf# .xf# Oscillator startup (.ENVOSC) .printev# .ev# .LIN analysis .PRINT output: .printac#; S/noise output: .sc#, .SnP, .citi# .PROBE output: .ac#; S/noise output: .sc#, .SnP, .citi# Phase Noise (.PHASENOISE) .printsnpn# .pn# .SN analysis .printsn# .sn# Transient analysis (.TRAN) .printtr# .tr# Using the CosmosScope Waveform Display CosmosScope has been enhanced to support viewing and processing of HSPICE RF output files. This section presents a basic overview of how to use CosmosScope to view HSPICE RF output. 12 ■ Type cscope on the UNIX command line to start the CosmosScope tool. ■ Choose File > Open > Plotfiles (or just press CTRL-O) to open the Open Plotfiles dialog. Use the Files of Type filter to find the HSPICE RF output file that you want to open. Table 3 on page 11 lists the HSPICE RF file types. When you open a file, its contents appear in the Signal Manager window. ■ The Signal Manager lists all open plot files. If you double-click a plot file name, a new window appears, showing the contents of that plot file. To plot one of the signals listed here in the active chart, double click on the signal label. ■ To create a new chart, use the File > New menu. Select either XY Graph, Smith Chart, or Polar Chart. You can also use the first three icons in the toolbar to create new chart windows. HSPICE® RF User Guide Z-2007.03 Chapter 2: Getting Started Using the CosmosScope Waveform Display ■ ■ To display the Signal Menu, right-click a signal label in a chart. Using this menu, you can change how signals look, delete signals, or move signals from one chart panel to another. • Use the Attributes menu item to control how the signal looks. • Use the Stack Region menu to move signals. You can move a signal to a new panel or an existing panel. The existing panels are named “Analog 0”, “Analog 1”, and so on; “Analog 0” is the bottom panel on a chart. • Use the To Time Domain command to convert a histogram plot (for example, from a .hb0 file) to a time domain signal. Right-click a horizontal or vertical axis to control an axis. Using the Axis Attributes dialog, you can use the Axis Menu to configure the axis precisely. • Use the Range submenu to zoom in or out. • Use the Scale submenu to switch between linear and logarithmic scales. • Lock Out New Signals creates an independent axis when you create a new panel. • Display Range Slider displays a region next to the axis. Click in that region to pan the display right, left, up, or down. ■ To zoom in and out, use the Axis Attributes dialog, the zoom buttons on the tool bar, or the mouse directly on the chart window. ■ To attach a marker to a signal, click on a signal label, then click the Vertical Marker or Horizontal Marker icons in the tool bar. You can use the mouse to drag the marker along the signal to see the signal’s precise value at different points. ■ Choose Tools > Calculator to open the Waveform Calculator tool. This tool can be used to generate new waveforms from existing ones. It is described in detail in the CosmosScope User Guide. The waveform calculator has no RF-specific features. ■ Tools > Measurement opens the Measurement Tool. Three RF measurements have been added, under the RF submenu of the measurement selection menu: • 1db compression point (1DB CP). • IIP3/OIP3. HSPICE® RF User Guide Z-2007.03 13 Chapter 2: Getting Started Using the CosmosScope Waveform Display • ■ 14 Spurious free dynamic range (SFDR). Tools > RF Tool opens the RF Tool, which generates contour plots on Smith or Polar charts. In HSPICE RF, the plotfile must be a file with a .sc# extension that a .LIN command generates. HSPICE RF automatically finds the S parameter and noise parameter data in the .sc# file, and uses it to generate noise, gain, and stability circles. HSPICE® RF User Guide Z-2007.03 3 HSPICE RF Tutorial 3 Provides a quick-start tutorial for users new to HSPICE RF. This tutorial assumes you are familiar with HSPICE and general HSPICE syntax, but new to RF analysis features. The most basic RF analysis features are presented here, using simple examples. The end of this chapter contains a listing of HSPICE RF demonstration files available for your use when you have access to the HSPICE RF installation directory. This tutorial covers the following examples: ■ Example 1: Using .LIN Analysis for a NMOS Low Noise Amplifier ■ Example 2: Using HB Analysis for a Power Amplifier ■ Example 3: Using HB Analysis for an Amplifier ■ Example 4: Using HBOSC Analysis for a Colpitts Oscillator ■ Example 5: Using HBOSC Analysis for a CMOS GPS VCO ■ Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer ■ Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator Example 1: Using .LIN Analysis for a NMOS Low Noise Amplifier The .LIN command simplifies the calculation of linear multi-port transfer parameters and noise parameters. In the LIN analysis, Port (P) elements are used to specify port numbers and their characteristic impedances. The analysis automatically computes the frequency-dependent complex transfer coefficients between ports. The result is a convenient means to get scattering parameters, noise parameters, stability parameters, and gain coefficients. The .LIN command renders obsolete the .NET command. The output from the .LIN HSPICE® RF User Guide Z-2007.03 15 Chapter 3: HSPICE RF Tutorial Example 1: Using .LIN Analysis for a NMOS Low Noise Amplifier command is saved in the *.sc0 file format that can, in turn, be referenced as a model file for the new S-parameter element. To set up a linear transfer parameter analysis, the HSPICE input netlist must contain: ■ Use the .AC command to activate small-signal AC analysis, and to specify a frequency sweep. Also, use the .AC command to specify any other parameter sweeps of interest. ■ Use the .LIN command with the .AC command to activate small-signal linear transfer analysis. The .AC command specifies the base frequency sweep for the LIN analysis. The LIN analysis automatically performs multiple AC and NOISE analyses, as needed to compute all complex signal transfer parameters. ■ The necessary number of port (P) elements, numbered sequentially beginning with one to define the terminals of the multi-port network. For example, a two-port circuit must contain two port elements with one listed as port=1 and the other as port=2. The port elements define the ordering for the output quantities from the .LIN command (for example, the terminals for port=1 are used for S11, Y11, and Z11 measurements). Much of the LIN analysis is automated so the HSPICE input netlist often does not require the following: ■ AC signal sources. The .LIN command computes transfer parameters between the ports with no additional AC sources needed. ■ DC sources. You can analyze a purely passive circuit without adding sources of any kind. The following tutorial example shows how to set up a LIN analysis for an NMOS low noise amplifier circuit. This netlist is shipped with the HSPICE RF distribution as gsmlna.sp and is available in the directory: $<installdir>/demo/hspicerf/examples. 16 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 1: Using .LIN Analysis for a NMOS Low Noise Amplifier ** NMOS 0.25um Cascode LNA for GSM applications ** setup for s-parameter and noise parameter measurements * Revision: 2.0, change to HB analysis and add measurements * 2 tone HB analysis, 1 tone as input, 1 tone as interfere Port element as power source, sweep input power ** .temp 27 .options post=2 .param Vdd=2.3 .global gnd ** ** Cascode LNA tuned for operation near 1 GHz ** M1 _n4 _n3 _n5 _n5 CMOSN l=0.25u w=7.5u + as=15p ad=15p ps=19u pd=19u m=80 M2 _n6 _n1 _n4 _n4 CMOSN l=0.25u w=7.5u + as=15p ad=15p ps=19u pd=19u m=80 M3 rfo _n6 gnd gnd CMOSN l=0.25u w=7.5u + as=15p ad=15p ps=19u pd=19u m=40 r1 _vdd _n6 400 l1 _n5 gnd l=0.9nH l2 rfin _n3 l=13nH vvb _n1 gnd dc=1.19 $ bias for common base device vvdd _vdd gnd dc=Vdd rfb rfo _n6 120 $ feedback ** ** 50 Ohm input port (incl. bias), 255 Ohm output port. ** P1 rfin gnd port=1 z0=50 dc = 0.595 $ input port includes DC bias P2 rfo _vdd port=2 z0=255 $ port doubles as pull-up resistor ** ** Measure s-parameters and noise parameters ** .AC DEC 50 100MEG 5G .LIN noisecalc=1 sparcalc=1 .PRINT S11(DB) S21(DB) S12(DB) S22(DB) NFMIN ** ** Approximate parameters for TSMC 0.25 Process (MOSIS run T17B) ** .MODEL CMOSN NMOS ( LEVEL = 49 3.1 TNOM = 27 TOX = 5.8E-9 +XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.3819327 +K1 = 0.477867 K2 = 2.422759E-3 K3 = 1E-3 +K3B = 2.1606637 W0 = 1E-7 NLX = 1.57986E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 HSPICE® RF User Guide Z-2007.03 17 Chapter 3: HSPICE RF Tutorial Example 1: Using .LIN Analysis for a NMOS Low Noise Amplifier +DVT0 +U0 +UC +AGS +KETA +RDSW +WR +XL +DWB +CIT +CDSCB +DSUB +PDIBLC2 +PSCBE1 +DELTA +PRT +KT1L +UB1 +WL +WWN +LLN +LWL +CGDO +CJ +CJSW +CJSWG +CF +PK2 * .END = = = = = = = = = = = = = = = = = = = = = = = = = = = = 0.5334651 289.1720829 2.841618E-11 0.2874763 -2.395348E-3 178.7751373 1 3E-8 4.613042E-9 0 0 0.0463218 4.422611E-3 7.982649E10 0.01 0 0 -7.61E-18 0 1 1 0 5.62E-10 1.641005E-3 4.179682E-10 3.29E-10 0 2.650965E-3 DVT1 UA VSAT B0 A1 PRWG WINT XW VOFF CDSC ETA0 PCLM PDIBLCB PSCBE2 RSH UTE KT2 UC1 WLN WWL LW CAPMOD CGSO PB PBSW PBSWG PVTH0 WKETA = = = = = = = = = = = = = = = = = = = = = = = = = = = = 0.7186877 -1.300598E-9 1.482651E5 -1.833193E-8 0 0.3774172 0 -4E-8 -0.0981658 2.4E-4 5.128492E-3 1.91946 -0.1 5.200359E-10 3.7 -1.5 0.022 -5.6E-11 1 0 0 2 5.62E-10 0.99 0.99 0.99 -8.385037E-3 7.293869E-3 DVT2 UB A0 B1 A2 PRWB LINT DWG NFACTOR CDSCD ETAB PDIBLC1 DROUT PVAG MOBMOD KT1 UA1 AT WW LL LWN XPART CGBO MJ MJSW MJSWG PRDSW LKETA = = = = = = = = = = = = = = = = = = = = = = = = = = = = -0.5 2.3082E-18 1.6856991 -1E-7 0.4177975 -0.2 1.88839E-8 -1.2139E-8 1.2032376 0 6.18609E-4 1 0.9817908 9.31443E-3 1 -0.11 4.31E-9 3.3E4 0 0 1 0.5 1E-12 0.4453094 0.3413857 0.3413857 -10 -6.070E-3) A LIN analysis also includes the following: ■ .LIN command: .LIN noisecalc=1 sparcalc=1 This invokes a LIN analysis and activates noise calculations and S parameter output files. ■ Two port elements: P1 rfin gnd port=1 z0=50 dc=0.595 Specifies that an input port is assumed between terminals rfin and ground, that it is has a 50 ohm termination, and it has a built-in DC bias of 0.595 V. The output (second) port is: 18 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 2: Using HB Analysis for a Power Amplifier P2 rfo _vdd port=2 z0=255 This syntax specifies that the output port is between terminals rfo and _vdd, and is being used as a pull up resistor with impedance of 255 ohms. ■ A .PRINT command for plotting the output S parameters in dB and the noise figure minimum. To run this netlist, type the following command: hspicerf gsmlna.sp This produces two output files, named gsmlna.sc0 and gsmlna.printac0, containing the S-parameter and noise parameter results, and the requested PRINT data. To view the output: 1. Type cscope to invoke CosmosScope. 2. Open gsmlna.sc0 in the File > Open > Plotfiles dialog. (Be sure to change the “Files of Type…” filter to find the sc0 file.) 3. To open a blank Smith chart, click the Smith chart icon, on the left side of the upper toolbar. 4. Using the signal manager, select the S(1,1) and S(2,2) signals under the S-Par heading from the gsmlna.sc0 file. You should see them plotted on the Smith chart. 5. To open a blank Polar chart, click the Polar chart icon on the left side of the upper toolbar. Now use the signal manager to select the S(2,1) signal under the S-Par heading to plot the complex gain of the LNA. 6. Open a blank X-Y plot. Use the signal manager to plot K (the Rollett stability factor) and Gas (the associated gain) under the Gain-Par heading, and NFMIN (the noise figure minimum) under the Noise-Par heading. Example 2: Using HB Analysis for a Power Amplifier The .HB command computes periodic steady-state solutions of circuits. This analysis uses the Harmonic Balance (HB) technique for computing such solutions in the frequency domain. The circuit can be driven by a voltage, power, or current source, or it may be an autonomous oscillator. The HB algorithm represents the circuit’s voltage and current waveforms as a Fourier series, that is, a series of sinusoidal waveforms. HSPICE® RF User Guide Z-2007.03 19 Chapter 3: HSPICE RF Tutorial Example 2: Using HB Analysis for a Power Amplifier To set up a periodic steady-state analysis, the HSPICE input netlist must contain: ■ A .HB command to activate the analysis. The .HB command specifies the base frequency (or frequencies, also called tones) for the analysis, and the number of harmonics to use for each tone. The .HB command can specify base tones so that the circuit solution is represented as a multi-dimensional Fourier series. The number of terms in the series are determined by the number of harmonics; more harmonics result in higher accuracy, but also longer simulation times and higher memory usage. ■ One or more signal sources for driving the circuit in HB analysis, if the circuit is driven. In the case of autonomous oscillator analysis, no signal source is required. Signal sources are specified using the HB keyword on the voltage or current source syntax. Power sources are specified by setting the power switch on voltage/current sources to 1; in this case, the source value is treated as a power value in Watts instead of a voltage or current. Optionally, the netlist can also contain a set of control option for optimizing HB analysis performance. The following example shows how to set up a Harmonic Balance analysis on an NMOS Class C Power Amplifier. The example compares transient analysis results to Harmonic Balance results. The following netlist performs both a transient and a Harmonic Balance analysis of the amplifier driven by a sinusoidal input waveform. The accurate option is set to ensure sufficient number of time points for comparison with HB. This example is included with the HSPICE RF distribution as pa.sp and is available in directory $<installdir>/demo/hspicerf/examples. 20 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 2: Using HB Analysis for a Power Amplifier .options POST accurate .param f0=950e6 PI=3.1415926 Ld=2e-9 Rload=5 Vin=3.0 .param Lin=0.1n Vdd=2 Cd='1.0/(4*PI*PI*f0*f0*Ld)' M1 drain gt 0 0 CMOSN L=0.35u W=50u AS=100p AD=100p PS=104u PD=104u M=80 Ls in gt Lin $ gate tuning Ld drain vdd Ld $ drain tuning Cd drain 0 Cd Cb drain out INFINITY $ DC block Rload out 0 Rload Vdd vdd 0 DC Vdd Vrf1 in 0 DC 'Vin/2.0' + SIN ('Vin/2' 'Vin/2' 'f0' 0 0 90) + HB 'Vin/2' 0.0 1 1 .hb tones=f0 nharms=10 .tran 10p 10n .probe hb p(Rload) .probe tran p(Rload) .include cmos49_model.inc .end An HB analysis uses the following: ■ An .HB command: .hb tones=f0 nharms=10 This invokes a single tone HB analysis with base frequency 950 mHz and 10 harmonics. ■ The HB source in Vrf1: HB ‘Vin/2’ 0.0 1 1. This creates a sinusoidal waveform matching the transient analysis one. The amplitude is Vin/2=1.5 V, and it applies to the first harmonic of the first tone, 950 MHz. ■ A .PROBE command for plotting the output power: .probe hb p(Rload) To run this netlist, type the following command: hspicerf pa.sp This produces two output files named pa.tr0 and pa.hb0, containing the transient and HB output, respectively. To view and compare the output: 1. Type cscope to invoke CosmosScope. HSPICE® RF User Guide Z-2007.03 21 Chapter 3: HSPICE RF Tutorial Example 3: Using HB Analysis for an Amplifier 2. To open both files, use the File > Open > Plotfiles dialog. (Be sure to change the “Files of Type…” filter to find the hb0 file.) 3. Using the signal manager, view the v(out) signals from the pa.tr0 file. A time domain waveform appears. 4. View the v(out) signal from the pa.hb0 file. This should be a histogram with lines at 950MHz, and multiples thereof, up to 9.5GHz. 5. Right-click on the waveform label for v(out) from the pa.hb0 file, and choose To Time-Domain. 6. Change the X-End(sec) value to 10n. 7. Click OK to accept the default interval value. You should now see a new waveform called timedomain(v(out)). 8. Left-click on the timedomain(v(out)) label, hold, and drag the signal to the plot containing v(out). This should overlay the v(out) and timedomain(v(out)) signals on the same panel. Zoom into the transitions to see the slight differences between the waveforms. Example 3: Using HB Analysis for an Amplifier This example takes the LNA circuit of Example 1 and performs a simulation using two closely spaced steady-state tones to study the compression and third order distortion properties of the amplifier. The example file gsmlnaIP3.sp is located at: /<install_dir>/demo/hspicerf/examples/ 22 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 3: Using HB Analysis for an Amplifier ** ** NMOS 0.25um Cascode LNA for GSM applications ** Test bench setup for two-tone power sweep in dBm ** to extract IP3. ** .temp 27 .options post=2 .param Vdd=2.3 .global gnd .param Pin:dBm=-30.0 .param Pin=Pin:dBm .param Pin:W='1.0e-3*pwr(10.0,Pin/10.0)' $ Change to Watts for sources ** ** Cascode LNA tuned for operation near 1 GHz ** M1 _n4 _n3 _n5 _n5 CMOSN l=0.25u w=7.5u as=15p ad=15p ps=19u pd=19u m=80 M2 _n6 _n1 _n4 _n4 CMOSN l=0.25u w=7.5u as=15p ad=15p ps=19u pd=19u m=80 M3 rfo _n6 gnd gnd CMOSN l=0.25u w=7.5u as=15p ad=15p ps=19u pd=19u m=40 r1 _vdd _n6 400 l1 _n5 gnd l=0.9nH l2 rfin _n3 l=13nH $ 0.65n vvb _n1 gnd dc=1.19 $ bias for common base device vinb rfinb gnd dc=0.595 lchk rfin rfinb INFINITY $ Choke cblk rfin rfind INFINITY $ DC block vvdd _vdd gnd dc=Vdd rfb rfo _n6 120 $ feedback ** ** ** Two-tone input source (DC blocked at this point) ** Vin rfind gnd dc=0 power=1 z0=50 $ 50 Ohm src + HB Pin:W 0 1 1 $ tone 1 + HB Pin:W 0 1 2 $ tone 2 Rload rfo _vdd R=255 ** ** HB test bench to measure IP3 and IP2 ** .HB tones=900MEG,910MEG nharms=11 11 intmodmax=7 + SWEEP Pin:dBm -50.0 0.0 2.0 .print HB P(Rload) P(Rload)[1,0] P(Rload)[2,0] P(Rload)[2,-1] .probe HB P(Rload) P(Rload)[1,0] P(Rload)[2,0] P(Rload)[2,-1] ** ** Approximate parameters for MOSIS 0.25um process (run T17B) ** HSPICE® RF User Guide Z-2007.03 23 Chapter 3: HSPICE RF Tutorial Example 3: Using HB Analysis for an Amplifier .MODEL CMOSN NMOS( LEVEL = 49 +VERSION = 3.1 TNOM = 27 TOX = 5.8E-9 +XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.3819327 +K1 = 0.477867 K2 = 2.422759E-3 K3 = 1E-3 +K3B = 2.1606637 W0 = 1E-7 NLX = 1.579864E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 +DVT0 = 0.5334651 DVT1 = 0.7186877 DVT2 = -0.5 +U0 = 289.1720829 UA = -1.300598E-9 UB = 2.308197E-18 +UC = 2.841618E-11 VSAT = 1.482651E5 A0 = 1.6856991 +AGS = 0.2874763 B0 = -1.833193E-8 B1 = -1E-7 +KETA = -2.395348E-3 A1 = 0 A2 = 0.4177975 +RDSW = 178.7751373 PRWG = 0.3774172 PRWB = -0.2 +WR = 1 WINT = 0 LINT = 1.888394E-8 +XL = 3E-8 XW = -4E-8 DWG = -1.213938E-8 +DWB = 4.613042E-9 VOFF = -0.0981658 NFACTOR = 1.2032376 +CIT = 0 CDSC = 2.4E-4 CDSCD = 0 +CDSCB = 0 ETA0 = 5.128492E-3 ETAB = 6.18609E-4 +DSUB = 0.0463218 PCLM = 1.91946 PDIBLC1 = 1 +PDIBLC2 = 4.422611E-3 PDIBLCB = -0.1 DROUT = 0.9817908 +PSCBE1 = 7.982649E10 PSCBE2 = 5.200359E-10 PVAG = 9.314435E-3 +DELTA = 0.01 RSH = 3.7 MOBMOD = 1 +PRT = 0 UTE = -1.5 KT1 = -0.11 +KT1L = 0 KT2 = 0.022 UA1 = 4.31E-9 +UB1 = -7.61E-18 UC1 = -5.6E-11 AT = 3.3E4 +WL = 0 WLN = 1 WW = 0 +WWN = 1 WWL = 0 LL = 0 +LLN = 1 LW = 0 LWN = 1 +LWL = 0 CAPMOD = 2 XPART = 0.5 +CGDO = 5.62E-10 CGSO = 5.62E-10 CGBO = 1E-12 +CJ = 1.641005E-3 PB = 0.99 MJ = 0.4453094 +CJSW = 4.179682E-10 PBSW = 0.99 MJSW = 0.3413857 +CJSWG = 3.29E-10 PBSWG = 0.99 MJSWG = 0.3413857 +CF = 0 PVTH0 = -8.385037E-3 PRDSW = -10 +PK2 = 2.650965E-3 WKETA = 7.293869E-3 LKETA = 6.070221E-3 ) * .END First, notice that we have defined variables that allow power to be swept in dBm units. .param Pin:dBm=-30.0 .param Pin=Pin:dBm .param Pin:W='1.0e-3*pwr(10.0,Pin/10.0)' 24 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 3: Using HB Analysis for an Amplifier References to sources must use SI units in conjunction with the previous equation to convert from dBm to Watts. The colon (:) is used as a labeling convenience. Second, a voltage source element is used as a two-tone power source by setting the power flag and a source impedance of 50 ohms is specified. The HB keyword is used to identify the amplitude (interpreted in Watts with the power flag set), phase, harmonic index, and tone index for each tone. Vin rfind gnd dc=0 power=1 z0=50 $ 50 Ohm src + HB Pin:W 0 1 1 $ tone 1 + HB Pin:W 0 1 2 $ tone 2 Third, the .HB command designates the frequencies of the two tones and establishes the power sweep using the dBm power variable. The intmodmax parameter has been set to 7 to include intermodulation harmonic content up to 7th order effects. .HB tones=900MEG,910MEG nharms=11 intmodmax=7 + SWEEP Pin:dBm -50.0 0.0 2.0 Last, the HSPICE RF ability to specify specific harmonic terms is used in the .PRINT and .PROBE statements to pull out the signals of particular interest. Notice the three different formats: .PRINT HB P(Rload) This reference dumps a complete spectrum in RMS Watts for the power across resistor Rload. .PRINT HB P(Rload)[1,0] This reference selectively dumps the power in resistor Rload at the first harmonic of the 1st tone. .PRINT HB P(Rload)[2,-1] This reference selectively dumps the power in resistor Rload at the 3rd intermodulation product frequency (890 MHz). To run this simulation, type the following line at the command line: hspicerf gsmlnaIP3.sp Viewing Results using CosmoScope For this analysis, the .print statement will generate a<design_name>.printhb0 file. Assume you want to find out the output power through the load resistor at the first tone when the input power is 0.1mW HSPICE® RF User Guide Z-2007.03 25 Chapter 3: HSPICE RF Tutorial Example 3: Using HB Analysis for an Amplifier To view the file: 1. Click the 4. Analysis button and then click on the Print tab. 2. Click the 3. Simulation button. 3. Invoke CosmosScope by clicking on the Waveform button. 4. Choose File > Open > Plotfiles to open the <design_name>.hb0 file. (Be sure to select HSPICERF (*.hb*, *.pn*, *.hr*, *.jt*) from the Files of type pulldown to find the <design_name>.hb0 file.) 5. Plot the signals Pr(rload) [1,0], Pr(rload) [2,0] and Pr(rload) [2 -1] on top of each other. The X-axis will be the input power and the Y-axis will be the output power. Result: CosmosScope will display the input and output power in dBm. But, there will be a (W) or (Watt) after the dBm label, this is incorrect. 6. To measure the 1dB compression point of the amplifier, open the measurement tool by clicking on the caliper icon at the bottom tool bar. Use the down arrow at the end of the Measurement field and select RF and P1dB. The PowerOut field should contain the Pr(rload):(1,0) trace. 7. Select a PowerIn value from the list.(The power value should be as large as possible, but still well within the linear range of the amplifier.) Try -25dbm. 8. Click the Apply button. Result: CosmoScope will show the linear gain of the amplifier and the 1dBcompression point. 9. The 3rd order intercept point is also measured by using the measurement tool. Use the down arrow at the end of the Measurement field and select RF and IP3/SFDR. The PowerOut1 field should contain the Pr(rload):(1,0) trace and the PowerOut3 field should contain the Pr(rload):(2, -1) trace. 10. Select a PowerIn value from the list. (The power value should be a value that is as large as possible but, still well within the linear range of the amplifier.) Try -25dbm. 11. Click Apply. Result: CosmosScope will show the 3rd order intercept point of the amplifier. 26 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 3: Using HB Analysis for an Amplifier Device Model Cards The following is an NMOS model in cmos49_model.inc file used in the power amplifier example. It is available in directory $<installdir>/demo/hspicerf/ examples. .MODEL CMOSN NMOS (LEVEL = 49 +VERSION = 3.1 TNOM = 27 TOX = 7.9E-9 +XJ = 1.5E-7 NCH = 1.7E17 VTH0 = 0.5047781 +K1 = 0.5719698 K2 = 0.0197928 K3 = 33.4446099 +K3B = -3.1667861 W0 = 1E-5 NLX = 2.455237E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 +DVT0 = 2.8937881 DVT1 = 0.6610934 DVT2 = -0.0446083 +U0 = 421.8714618 UA = -1.18967E-10 UB = 1.621684E-18 +UC = 3.422111E-11 VSAT = 1.145012E5 A0 = 1.119634 +AGS = 0.1918651 B0 = 1.800933E-6 B1 = 5E-6 +KETA = 3.313177E-3 A1 = 0 A2 = 1 +RDSW = 984.149934 PRWG = -1.133763E-3 PRWB = -7.19717E-3 +WR = 1 WINT = 9.590106E-8 LINT = 1.719803E-8 +XL = -5E-8 XW = 0 DWG = -2.019736E-9 +DWB = 6.217095E-9 VOFF = -0.1076921 NFACTOR = 0 +CIT = 0 CDSC = 2.4E-4 CDSCD = 0 +CDSCB = 0 ETA0 = 0.0147171 ETAB = -7.256296E-3 +DSUB = 0.3377074 PCLM = 1.1535622 PDIBLC1 = 2.946624E-4 +PDIBLC2= 4.171891E-3 PDIBLCB = 0.0497942 DROUT = 0.0799917 +PSCBE1 = 3.380501E9 PSCBE2 = 1.69587E-9 PVAG = 0.4105571 +DELTA = 0.01 MOBMOD = 1 PRT = 0 +UTE = -1.5 KT1 = -0.11 KT1L = 0 +KT2 = 0.022 UA1 = 4.31E-9 UB1 = -7.61E-18 +UC1 = -5.6E-11 AT = 3.3E4 WL = 0 +WLN = 1 WW = -1.22182E-15 WWN = 1.1657 +WWL = 0 LL = 0 LLN = 1 +LW = 0 LWN = 1 LWL = 0 +CAPMOD = 2 XPART = 0.4 CGDO = 3.73E-10 +CGSO = 3.73E-10 CGBO = 1E-11 CJ = 8.988141E-4 +PB = 0.8616985 MJ = 0.3906381 CJSW = 2.463277E-10 +PBSW = 0.5072799 MJSW = 0.1331717 PVTH0 = -0.0143809 +PRDSW = -81.683425 WRDSW = -107.8071189 PK2 = 1.210197E-3 +WKETA = -1.00008E-3 LKETA = -6.1699E-3 PAGS = 0.24968) The following is the BJT model file, bjt.inc used in oscillator example. It is available in directory $<installdir>/demo/hspicerf/examples. HSPICE® RF User Guide Z-2007.03 27 Chapter 3: HSPICE RF Tutorial Example 4: Using HBOSC Analysis for a Colpitts Oscillator * RF Wideband NPN Transistor die SPICE MODEL .MODEL RF_WB_NPN NPN + IS = 1.32873E-015 BF = 1.02000E+002 + NF = 1.00025E+000 VAF = 5.19033E+001 + EG = 1.11000E+000 XTI = 3.00000E+000 + CJE = 2.03216E-012 VJE = 6.00000E-001 + MJE = 2.90076E-001 TF = 6.55790E-012 + XTF = 3.89752E+001 VTF = 1.09308E+001 + ITF = 5.21078E-001 CJC = 1.00353E-012 + VJC = 3.40808E-001 MJC = 1.94223E-001 Example 4: Using HBOSC Analysis for a Colpitts Oscillator This section demonstrates HSPICE RF oscillator analysis using a single transistor oscillator circuit. Oscillator analysis is an extension of Harmonic Balance in which the base frequency itself is an unknown to be solved for. In oscillator analysis, the user supplies a guess at the base frequency, and no voltage or current source stimulus is needed. To activate oscillator analysis, include a .HBOSC command with: ■ The TONE parameter set to a guess of the oscillation frequency. ■ The PROBENODE parameter set to identify an oscillating node or pair of nodes. Always specify a pair of nodes; if only one node oscillates, specify ground as the second node. To speed up the simulation, also supply a guess at the magnitude of the oscillating voltage across these nodes. ■ The FSPTS parameter set to a frequency range and number of search points. When you set FSPTS, HSPICE RF precedes the HBOSC analysis with a frequency search in the specified range to obtain an optimal initial guess for the oscillation frequency. This can accelerate the HB oscillator convergence. In conjunction with oscillator analysis, HSPICE RF can perform phase noise analysis. Phase noise analysis measures the effect of transistor noise on the oscillator frequency. Phase noise analysis is activated using the .PHASENOISE command; this command sets a set of frequency points for phase noise analysis. The .PRINT and .PROBE commands can be used to output phase noise values. The following netlist, osc.sp, simulates an oscillator, and performs phase noise analysis. This example is included with the HSPICE RF distribution as pa.sp and is available in directory $<installdir>/demo/hspicerf/examples. Use the .HBOSC command with the PROBENODE and FSPTS parameters set. 28 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 4: Using HBOSC Analysis for a Colpitts Oscillator PROBENODE=emitter,0,4.27 Identifies the emitter node as an oscillating node, and provides a guess value of 4.27 volts for the oscillation amplitude at the emitter node. FSPTS=40,9e6,1.1e7 Causes an initial frequency search using 40 equally-spaced points between 9 and 11 MHz. In the .PHASENOISE, .PRINT, and .PROBE commands: .PHASENOISE V(emitter) dec 10 10k 1meg Runs phase noise analysis at the specified offset frequencies, measured from the oscillation carrier frequency. The frequency points specified here are on a logarithmic scale, 10 points per decade, 10 kHz to 1 MHz. ■ .PROBE PHASENOISE PHNOISE and the similar .PRINT command instruct HSPICE RF to output phase noise results to the osc.pn0 and osc.printpn0 files. ** ** Uses emitter resistor limiting to keep output sinusoidal. ** Output can be taken at the emitter (eml node). ** *--------------------------------------------------------* Options for Oscillator Harmonic Balance Analysis... * .OPTIONS post sim_accuracy=100 hbsolver=0 *--------------------------------------------------------* Bias NPN transistor for 5V Vce, 10mA Ic * Emitter follower Colpitts design Vcc collector 0 9V Q1 collector base emitter emitter RF_WB_NPN Re1 emitter eml 100 RLoad eml 0 300 Rb1 collector base 4300 Rb2 base 0 5600 * *--------------------------------------------------------* Capacitive feedback network Ce 0 eml 100pF Cfb base eml 100pF Cbb base bb 470pF Lb bb 0 6uH *--------------------------------------------------------- HSPICE® RF User Guide Z-2007.03 29 Chapter 3: HSPICE RF Tutorial Example 4: Using HBOSC Analysis for a Colpitts Oscillator * Simulation control for automated oscillator analysis * .HBOSC tones=1.0e7 nharms=15 +PROBENODE=emitter,0,4.27 +FSPTS=40,9.e6,1.1e7 * .PHASENOISE V(emitter) DEC 10 10K 1MEG +METHOD=0 CARRIERINDEX=1 * .print hbosc vm(eml) vp(eml) vr(emitter) vi(emitter) .print hbosc vm(emitter) vp(emitter) P(Rload) .print phasenoise phnoise .probe phasenoise phnoise .probe hbosc v(emitter) v(eml) .include bjt.inc .END After you run this netlist, examine the osc.printhb0 file. ■ At the top is the oscillator frequency (about 10.14 MHz) and the .PRINT HBOSC output. ■ The first 2 lines show that the eml node oscillates around 3V with an amplitude of about 2.85V. ■ The emitter node oscillates around 4V with an amplitude of about 4.27V. Also examine the osc.printpn0 file, which contains the phase noise results in text form. You can view the osc.hb0 and osc.pn0 files in CosmosScope. 1. To start CosmosScope, type cscope. 2. Use the File > Open > Plotfiles dialog to open osc.hb0. Remember to set the file type filter to HSPICE RF HB (*.hb*). 3. From the signal manager, double click on v(emitter) to see that node’s spectrum. 4. Right-click on the v(emitter) label in the chart, and choose “To Time Domain” to create a time domain waveform. 5. To accept the defaults for range and interval, click OK. You should see an oscillating time domain waveform. To run a transient simulation for comparison: 1. Use the .TRAN 1n 10u command. 30 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO 2. Add ic=10n to the Lb inductor. The resulting waveforms should be the same as those from HB oscillator analysis. Example 5: Using HBOSC Analysis for a CMOS GPS VCO This second oscillator analysis example involves two negative resistance oscillators coupled at 90 degrees. MOS capacitors are used as varactors. This VCO topology is common for GPS applications and produces quadrature LO outputs near 1550 MHz. The purpose of this example is to generate the VCO tuning curve (output level and frequency as a function of tuning voltage) as well as its phase noise characteristics as a function of tuning voltage. As in previous examples, the oscillator analysis is activated using the .HBOSC command: ■ The TONE parameter sets an approximate oscillation frequency (near 1550 MHz). ■ The NHARMS parameter sets the harmonic content to 11th order. ■ The PROBENODE parameters identify the drain pins across the first oscillator section as the pair of oscillating nodes. This is a differential oscillator, and the approximate value for this differential amplitude is 6.1 V. ■ The FSPTS parameters set the search frequency range between 1500 and 1600 MHz. ■ The SWEEP parameters set a tuning voltage sweep from 2.0 to 3.2 V. The following example is based on demonstration netlist gpsvco.sp, which is available in directory $<installdir>/demo/hspicerf/examples. This netlist simulates the oscillator schematic shown in Figure 1 and performs phase noise analysis. HSPICE® RF User Guide Z-2007.03 31 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO ** ** NMOS IC Quadrature VCO circuit for GPS local oscillator ** ** Twin differential negative resistance VCOs using NMOS ** transistors for varactors, coupled to produce quadrature ** resonances. ** Design based on 0.35um CMOS process. ** ** References: ** >P. Vancorenland and M.S.J. Steyaert, "A 1.57-GHz fully ** integrated very low-phase-noise quadrature VCO," ** IEEE Trans. Solid-State Circuits, May 2002, pp.653-656. ** >J. van der Tang, P. van de Ven, D. Kasperkovitz, and A. Roermund, ** "Analysis and design of an optimally coupled 5-GHz quadrature ** LC oscillator," IEEE Trans. Solid-State Circuits, May 2002, ** pp.657-661. ** >F. Behbahani, H. Firouzkouhi, R. Chokkalingam, S. Delshadpour, ** A. Kheirkhani, M. Nariman, M. Conta, and S. Bhatia, ** "A fully integrated low-IF CMOS GPS radio with on-chip analog ** image rejection," IEEE Trans. Solid-State Circuits, Dec. 2002, ** pp. 1721-1727. ** ** Setup for Harmonic Balance Analysis ** ** Oscillation Frequency: ~ 1575 MHz (GPS L1 frequency) ** Amplitude: ~5 Volts peak-to-peak (zero to 5V) ** Vdd: 2.5 V ** ** HSPICE Simulation Options: *.option delmax=1n ACCURATE LIST NODE ** ** HSPICE RF Simulation Options : .option sim_accuracy=10 ** *.option savehb=’a.hbs’ loadhb=’a.hbs’ .option POST .param Vtune=2.0 $ Failures: vtune=1 .param Cval=0.2p *--------------------------------Vtune vc gnd DC Vtune Vdd vdd gnd 2.5 *--------------------------------* First oscillator section ** Low-Q resonator with Vdd at center tap of inductors R1a IP ri 100k $ These R’s set the Q R1b ri IN 100k L1 IP vdd 16.5nH 32 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO L2 vdd IN 16.5nH Cc1 IP gnd Cval $ I to Q Cc2 IN gnd Cval $ -I to Q ** Differential fets M1 IP IN cs gnd NMOS l=0.35u w=15u M2 IN IP cs gnd NMOS l=0.35u w=15u ** Bias fet - bias at Vdd -- too high? Mb cs vdd gnd gnd NMOS l=0.35u w=15u ** fets used as varactors Mt1 vc IP vc gnd NMOS l=0.35u w=2u M=50 Mt2 vc IN vc gnd NMOS l=0.35u w=2u M=50 *--------------------------------** Second oscillator section ** Low-Q resonator with Vdd at center tap of inductors R1a_b QP ri_b 100k $ These R’s set the Q R1b_b ri_b QN 100k L1_b QP vdd 16.5nH L2_b vdd QN 16.5nH Cc1_b QP gnd Cval $ -Q to -I Cc2_b QN gnd Cval $ -Q to I ** Differential fets M1_b QP QN cs_b gnd NMOS l=0.35u w=15u M2_b QN QP cs_b gnd NMOS l=0.35u w=15u ** Bias fet - bias at Vdd -- too high? 2nd in parallel Mb_b cs_b vdd gnd gnd NMOS l=0.35u w=15u ** fets used as varactors Mt1_b vc QP vc gnd NMOS l=0.35u w=2u M=50 Mt2_b vc QN vc gnd NMOS l=0.35u w=2u M=50 * *------------------------------* Differentiators Coupling transistors for quadrature * .param Cdiff=0.14p difMsize=50u vidiff dbias gnd 1.25 viqdiff vdcdif gnd 1.75 Midiff1 dQP dbias gnd gnd NMOS l=0.35u w=difMsize Midiff2 dQN dbias gnd gnd NMOS l=0.35u w=difMsize Midiff3 dIN dbias gnd gnd NMOS l=0.35u w=difMsize Midiff4 dIP dbias gnd gnd NMOS l=0.35u w=difMsize Cdiff1 dQP QP Cdiff Cdiff2 dQN QN Cdiff Cdiff3 dIN IN Cdiff Cdiff4 dIP IP Cdiff Mc_QP1 IP vdcdif dQP gnd NMOS l=0.35u w=difMsize Mc_QN2 IN vdcdif dQN gnd NMOS l=0.35u w=difMsize Mc_QN3 QP vdcdif dIN gnd NMOS l=0.35u w=difMsize Mc_QP4 QN vdcdif dIP gnd NMOS l=0.35u w=difMsize *------------------------------- HSPICE® RF User Guide Z-2007.03 33 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO * Transient Analysis Test Bench * * stimulate oscillation with 2mA pulse *iosc IP IN PULSE ( 0 2m .01n .01n .01n 10n 1u ) *.probe tran v(IP) v(IN) *.print tran v(IP) v(IN) *.TRAN .01n 10n *-----------------------------* Harmonic Balance Test Bench * .sweepblock vtune_sweep + 0 5 0.2 + 2 3 0.1 .HBOSC tones=1550e6 nharms=12 + PROBENODE=IP,QN,4 + sweep Vtune sweepblock=vtune_sweep ** .phasenoise dec 10 100 1e7 .print phasenoise phnz .probe phasenoise phnz .print hb v(IP,IN) v(IP,IN)[1] v(QP,QN) v(QP,QN)[1] .probe hb v(IP,IN) v(IP,IN)[1] v(QP,QN) v(QP,QN)[1] .probe hb hertz[1][1] * * NMOS Device from MOSIS 0.35um Process * * BSIM3 VERSION 3.1 PARAMETERS * * DATE: Mar 8/00 * LOT: n9co WAF: 07 * Temperature_parameters=Default * .MODEL NMOS NMOS ( LEVEL = 49 +VERSION = 3.1 TNOM = 27 TOX = 7.9E-9 +XJ = 1.5E-7 NCH = 1.7E17 VTH0 = 0.5047781 +K1 = 0.5719698 K2 = 0.0197928 K3 = 33.4446099 +K3B = -3.1667861 W0 = 1E-5 NLX = 2.455237E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 +DVT0 = 2.8937881 DVT1 = 0.6610934 DVT2 = -0.0446083 +U0 = 421.8714618 UA = -1.18967E-10 UB = 1.621684E-18 +UC = 3.422111E-11 VSAT = 1.145012E5 A0 = 1.119634 +AGS = 0.1918651 B0 = 1.800933E-6 B1 = 5E-6 +KETA = 3.313177E-3 A1 = 0 A2 = 1 +RDSW = 984.149934 PRWG = -1.133763E-3 PRWB = -7.19717E-3 +WR = 1 WINT = 9.590106E-8 LINT = 1.719803E-8 +XL = -5E-8 XW = 0 DWG = -2.019736E-9 +DWB = 6.217095E-9 VOFF = -0.1076921 NFACTOR = 0 +CIT = 0 CDSC = 2.4E-4 CDSCD = 0 34 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO +CDSCB = 0 ETA0 = 0.0147171 ETAB = -7.256296E-3 +DSUB = 0.3377074 PCLM = 1.1535622 PDIBLC1 = 2.946624E-4 +PDIBLC2 = 4.171891E-3 PDIBLCB = 0.0497942 DROUT = 0.0799917 +PSCBE1 = 3.380501E9 PSCBE2 = 1.69587E-9 PVAG = 0.4105571 +DELTA = 0.01 MOBMOD = 1 PRT = 0 +UTE = -1.5 KT1 = -0.11 KT1L = 0 +KT2 = 0.022 UA1 = 4.31E-9 UB1 = -7.61E-18 +UC1 = -5.6E-11 AT = 3.3E4 WL = 0 +WLN = 1 WW = -1.22182E-15 WWN = 1.1657 +WWL = 0 LL = 0 LLN = 1 +LW = 0 LWN = 1 LWL = 0 +CAPMOD = 2 XPART = 0.4 CGDO = 3.73E-10 +CGSO = 3.73E-10 CGBO = 1E-11 CJ = 8.988141E-4 +PB = 0.8616985 MJ = 0.3906381 CJSW = 2.463277E-10 +PBSW = 0.5072799 MJSW = 0.1331717 PVTH0 = -0.0143809 +PRDSW = -81.683425 WRDSW = -107.8071189 PK2 = 1.210197E-3 +WKETA = -1.00008E-3 LKETA = -6.1699E-3 PAGS = 0.24968 +AF = 1.0 KF = 1.0E-30 ) * .END Figure 1 HSPICE® RF User Guide Z-2007.03 VCO Schematic 35 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO The results of the analysis are displayed in Figure 2 on page 36, Figure 3 on page 37, and Figure 4 on page 38 using CosmosScope for VCO waveforms, tuning curves, and phase noise response. Figure 2 36 VCO Waveforms Output in CosmosScope HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 5: Using HBOSC Analysis for a CMOS GPS VCO Figure 3 HSPICE® RF User Guide Z-2007.03 VCO Tuning Curves Output in CosmosScope 37 Chapter 3: HSPICE RF Tutorial Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer Figure 4 VCO Phase Noise Response in CosmosScope Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer The example in this section shows how to use HSPICE RF to analyze a circuit driven by multiple input stimuli with different frequencies. Mixer circuits provide a typical example of this scenario: in this case, there might be two input signals (LO and RF), which are mixed to produce an IF output signal. In this case, HSPICE RF offers two options: 38 ■ Multi-tone HB analysis: specify the LO and RF base frequencies as two separate tones on the .HB command. ■ Periodic AC analysis (HBAC): if one of the inputs is a small-signal, you can use a faster linear analysis to analyze its effect. For example, if a mixer’s LO is a large signal, but RF is a small signal, a single-tone HB analysis using the LO frequency can be combined with HBAC in place of a 2-tone HB analysis. HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer To demonstrate both techniques, this example analyzes an ideal mixer built using behavioral elements. It is based on demonstration netlist mix_tran.sp, which is available in directory $<installdir>/demo/hspicerf/examples. * Ideal mixer example: transient analysis .OPTIONS POST vlo lo 0 1.0 sin (1.0 0.5 1.0g 0 0 90) rrf1 rf1 rf 1.0 g1 0 if cur='1.0*v(lo)*v(rf)' $ mixer element c1 0 if q='1.0e-9*v(lo)*v(rf)' $ mixer element rout if ifg 1.0 vctrl ifg 0 0.0 h1 out 0 vctrl 1.0 $ convert I to V rh1 out 0 1.0 vrf rf1 0 sin (0 0.001 0.8GHz 0 0 114) .tran 10p 10n .opt sim_accuracy=100 .end This example uses behavioral controlled current and charge sources to simulate a mixer. The LO signal is driven by a 0.5 Volt sinusoid at 1 GHz, and RF is driven by a 10mV signal at 800 MHz. The mixer output is the voltage at node out, v(out). Two-tone HB Approach To analyze this circuit using 2-tone HB, add: ■ HB source for LO: add HB 0.5 0 1 1 to the LO voltage source; this sets the amplitude to 0.5, no phase shift for the first harmonic of the first tone, which is 1 GHz. ■ HB source for RF: add HB 0.001 24 1 2 to the RF voltage source; this sets the amplitude to 0.001, 24 degrees phase shift for the first harmonic of the second tone (0.8 GHz). ■ An .HB command specifying both tones: .hb tones=1g 0.8g nharms=6 3; only a small number of harmonics is required to resolve the signals. The complete mix_hb.sp netlist for 2-tone HB analysis is then: HSPICE® RF User Guide Z-2007.03 39 Chapter 3: HSPICE RF Tutorial Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer * Ideal mixer example: 2-tone HB analysis .OPTIONS POST vlo lo 0 1.0 sin (1.0 0.5 1.0g 0 0 90) HB 0.5 0 1 1 rrf1 rf1 rf 1.0 g1 0 if cur='1.0*v(lo)*v(rf)' $ mixer element c1 0 if q='1.0e-9*v(lo)*v(rf)' $ mixer element rout if ifg 1.0 vctrl ifg 0 0.0 h1 out 0 vctrl 1.0 $ convert I to V rh1 out 0 1.0 vrf rf1 0 sin (0 0.001 0.8GHz 0 0 114) HB 0.001 24 1 2 .opt sim_accuracy=100 .hb tones=1g 0.8g nharms=6 3 .end This example is available in directory $<installdir>/demo/hspicerf/examples. HBAC Approach To analyze this circuit using HBAC, start with the 2-tone HB analysis setup, and modify it as follows: ■ Replace the RF HB signal with an HBAC signal: change HB 0.001 24 1 2 to HBAC 0.001 24; this deactivates the source for HB and activates it for HBAC with the same magnitude and phase. ■ Specify the frequency in the .HBAC command. ■ Change the .HB command to single tone: .HB tones=1g nharms=6 HBAC takes care of the second tone. ■ Add a .HBAC command .HBAC lin 1 0.8g 0.8g This command runs an analysis at a single frequency point, 0.8 GHz. In general, HBAC analysis can sweep the RF frequency over a range of values. The following is the complete mix_hbac.sp netlist for HBAC analysis of this simple mixer. This netlist also contains commands for performing periodic noise analysis. It is available in directory $<installdir>/demo/hspicerf/examples. 40 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer * Ideal mixer example: HBAC analysis .OPTIONS POST vlo lo 0 1.0 sin (1.0 0.5 1.0g 0 0 90) + HB 0.5 0 1 1 rrf1 rf1 rf 1.0 g1 0 if cur='1.0*v(lo)*v(rf)' $ mixer element c1 0 if q='1.0e-9*v(lo)*v(rf)' $ mixer element rout if ifg 1.0 vctrl ifg 0 0.0 h1 out 0 vctrl 1.0 $ convert I to V rh1 out 0 1.0 vrf rf1 0 sin (0 0.001 0.8GHz 0 0 114) + HBAC 0.001 24 .opt sim_accuracy=100 .hb tones=1g nharms=6 .hbac lin 1 0.8g 0.8g * Noise analysis .hbnoise v(out) rrf1 lin 40 0.1g 4g .print hbnoise onoise nf .probe hbnoise onoise nf .end Comparing Results After running all three netlists above, you will have generated 3 output files: ■ mix_tran.tr0 ■ mix_hb.hb0 ■ mix_hbac.hb0 You can compare the results of the 3 analyses in CosmosScope. 1. To run the netlists and start CosmosScope, type: hspicerf mix_tran.sp hspicerf mix_hb.sp hspicerf mix_hbac.sp cscope & 2. Open the mix_tran.tr0 file: choose File>Open>Plotfiles and select mix_tran.tr0. 3. To plot v(out), double-click v(out) in the signal manager. 4. Open the mix_hb.hb0 file: choose File>Open>Plotfiles and select mix_hb.hb0. HSPICE® RF User Guide Z-2007.03 41 Chapter 3: HSPICE RF Tutorial Example 6: Using Multi-Tone HB and HBAC Analyses for a Mixer You might need to change the “Files of Type…” filter to “HSPICERF HB (*.hb*)”. 5. Plot v(out) by double clicking v(out) in the signal manager. A histogram displays. 6. Open the mix_hbac.hb0 file: choose File>Open>Plotfiles and select mix_hbac.hb0. You might need to change the “Files of Type…” filter to “HSPICERF HBAC (*.hb*)”. 7. Plot v(out) by double clicking v(out) in the signal manager. You should see a histogram similar to the one from mix_hb.hb0. 8. Convert the HB and HBAC histograms to time domain. For each of the two v(out) histogram signals, right-click on the v(out) label and choose To Time Domain. Accept the default range and interval settings. Two new time domain waveforms should appear. 9. Overlay the three time domain plots. Right click on each “timedomain(v(out))” label, and choose Stack Region/Analog 0. The bottom panel should now display all three time domain signals. All three are almost indistinguishable from each other. You can also use HBAC to perform noise analysis on RF circuits by using the .HBNOISE command, which is included in the mix_hbac.sp netlist. ■ The .HBNOISE command invokes noise analysis, identifying an output node where the noise is measured, an input noise source (in this case, rrf1) which serves as a reference for noise figure computation, and a frequency sweep for the noise analysis. ■ The .PRINT and .PROBE hbnoise commands instruct HSPICE RF to save the output noise and noise figure at each frequency in the mix_hbac.printpn0 and mix_hbac.pn0 output files. This ideal mixer is noiseless, except for the resistors at the input and output. The mix_hbac.lis file contains detailed data on the individual noise source contributions of the resistors. You can view mix_hbac.printpn0 to see the output noise and noise figure at each frequency. In CosmosScope, you can view mix_hbac.pn0 to plot the output noise and noise figure data as a function of frequency. 42 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator Introduction While the Harmonic Balance (HB) algorithm represents the circuit's voltage and current waveforms as a Fourier series (a series of sinusoidal waveforms), the Shooting Newton (SN) algorithm provides analysis capability for digital logic circuits and RF components that require steady-state analysis, but operate with waveforms that tend to be square instead of sinusoidal. Simple examples of using the Shooting Newton analysis functions are presented in this section: ■ Driven Phase Frequency Example ■ Ring Oscillator Example Shooting Newton Analysis Setup To set up a time-domain, steady-state analysis, the HSPICE input netlist must contain: ■ An .SN command to activate the analysis. The .SN command specifies: • The expected period of the steady-state waveforms, which must match the period of any input waveforms. The period is specified in time domain units (seconds). Alternatively, you may specify a frequency in Hz. • A time resolution, which is analogous to the transient analysis (.TRAN) command’s TSTEP parameter and will affect the time step size selection. It also affects the number of frequency terms used in smallsignal analyses, such as periodic AC or noise analysis. The time resolution is typically specified in seconds but, alternatively, may be specified in the frequency domain as a number of harmonics. • A transient initialization time that is used by HSPICE RF to run a basic transient simulation of this length before attempting Newton-Raphson iterations to converge on a steady-state solution. This parameter is optional. If it is not specified, the specified period is used as the HSPICE® RF User Guide Z-2007.03 43 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator initialization time. The initial transient analysis is used for circuit stabilization before the steady state solution is found. Larger initialization values typically result in convergence that is more robust. ■ ■ For oscillator circuits, a .SNOSC command is used to activate the analysis. The .SNOSC command specifies: • The approximate frequency of oscillation specified either as a frequency (in Hertz) or as the time domain period. • The number of high frequency harmonics. Alternatively, a time resolution in seconds can be specified. • A transient initialization time that is used by HSPICE RF to run a basic transient simulation of this length before attempting Newton-Raphson iterations to converge on a steady state solution. This parameter is optional. If it is not specified, the period of the specified frequency of oscillation is used as the initialization time. For oscillators we recommend specifying a transient initialization time since the default initialization time is usually too short to effectively stabilize the circuit. • A node at which to probe for oscillation conditions. • If the tuning curve of a VCO is to be analyzed, the optional parameter MAXTRINITCYCLES can be specified. One or more signal sources for driving the circuit in SN analysis, if the circuit is driven. In the case of autonomous oscillator analysis, no signal source is required. The sources are required to be time domain sources and must match the period specified in the .SN command. Driven Phase Frequency Example This example demonstrates the Shooting Newton-based analysis of a driven phase-frequency detector. Extracted portions of the input file are presented below. The complete phasefreqdet.sp input file for this example is located in the following directory: $installdir/demo/hspicerf/examples/ During the analysis, the phase of the input signal is swept between 0 degrees and 90 degrees using five equally spaced steps. This enables us to measure the phase detector gain at the output load. We use the .SN command syntax that specifies the expected period of the steady-state waveforms as a frequency (0.5GHz) and the time resolution as the number of harmonics (127). 44 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator A periodic, time-varying AC noise analysis based on the Shooting Newton algorithm is performed using the .SNNOISE command. The .SNNOISE analysis requires an output node (v(lfin) where the noise is to be measured, an input noise source (Vref) which serves as the reference for the noise computation and, a frequency sweep for the noise analysis. Optionally, an index term can be defined. The index term specifies the output frequency band at which the noise is evaluated. For this case, we want to evaluate the low frequency noise of the phase frequency detector. The time-domain signals v(cfin), v(fin), v(pu) and v(pdn) and v(lfin) are be probed. The gain of the phase frequency detector can be found by probing the frequency domain value of v(lfin) at DC (frequency indices 0). * Phase Frequency Detector : : .global vdd gnd .options wl post * DC sources vsup vdd 0 DC 1.0 * Reference signal (sine wave) vref xin gnd DC 0 sin( 0.5 0.5 0.5g 0.0 0.0 0.0) * Input buffers (square up Ref sine wave) xfin1 xin fin1 inv xfin2 fin1 FIN inv3 * Compare signal (sine wave) vcRef cin gnd DC 0 sin( 0.5 0.5 0.5g 0.0 0.0 phase) $ phase shift * Input buffers (square up compare sine wave) xcfin1 cin cfin1 inv xcfin2 cfin1 cFIN inv3 * ** Phase/frequency detector xPFD cFIN FIN pdn pu phasedet ** Chargepump xCP LFIN Ibias pdn pu chargepump ** Bias voltage vIbias Ibias gnd 0.15 $ Sets charge pump bias! Rload LFIN 0 10Meg * Harmonic Balance Test Bench * .param NH=127 .param phase=0.0 $ phase shift in degrees .opt snaccuracy=30 .SN tone=0.5g nharms=NH SWEEP phase POI 5 0.0 22.5 45.0 67.5 90.0 .SNNOISE V(LFIN) Vref + DEC 21 100 10MEG $ offset frequency sweep + [0,1] $ Take low frequency noise HSPICE® RF User Guide Z-2007.03 45 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator * .probe .print .probe .probe .print .end sn v(fin) v(cfin) v(pu) v(pdn) v(lfin) i(vibias) snfd v(lfin) v(lfin) [0] snfd v(lfin) v(lfin) [0] SNNOISE ONOISE SNNOISE ONOISE Simulation Status Output During the simulation, the simulation status is displayed on the screen. In addition to the screen display, more detailed status, cpu time and memory usage information is also be written to the phasefreqdet.lis file. Parsing Loading Netlist Data Checking Compressing Simulation Time Domain RF Analysis Steady-State Time Domain Analysis will use the matrix-implicit gmres solver. starting Shooting Newton Sweep Shooting Newton Sweep: 0.0% PHASE = 0.000000 ( etc = 0.0 sec, ett = 0.0 sec ) Input period: 2e-09 begin circuit stabilization time 20% ... 40% ... 60% ... 80% ... 100% circuit stabilization time done ***************************************************** ********** Shooting-Newton iteration 1 ************** ***************************************************** 20% 40% 60% 80% 100% number of transient points: 276 start GMRES number of GMRES iterations: 3 current residual: 6.79374e-09 voltage residual: 0.000183225 : 46 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator : ***************************************************** ********** Shooting-Newton iteration 4 ************** ***************************************************** 20% ... 40% ... 60% ... 80% ... 100% number of transient points: 1471 start GMRES number of GMRES iterations: 3 current residual: 1.37423e-17 voltage residual: 2.12608e-13 20% ... 40% ... 60% ... 80% ... 100% Starting SNNOISE analysis ... TD-PAC, FFT-Noise Algorithm ... Using GMRES Solver 4% completed Estimated 4.6 Min Remaining 10% completed Estimated 3.8 Min Remaining 21% completed Estimated 3.2 Min Remaining 30% completed Estimated 2.8 Min Remaining 41% completed Estimated 2.4 Min Remaining 51% completed Estimated 119 Sec Remaining 60% completed Estimated 97 Sec Remaining 71% completed Estimated 72 Sec Remaining 80% completed Estimated 50 Sec Remaining 91% completed Estimated 24 Sec Remaining Finished SNNOISE-TDFD analysis (265.16 sec) Steady-State Time Domain has converged successfully in 3 iterations : HSPICE® RF User Guide Z-2007.03 47 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator : Finished SNNOISE-TDFD analysis (405.86 sec) Steady-State Time Domain has converged successfully in 4 iterations finished Shooting Newton Sweep (2200.5 sec) Shooting-Newton time = 2200.53 cpu sec Total Shooting-Newton memory = 228.86 Mbytes Viewing Results in CosmosScope To view the time-domain, phasefreqdet.sn0 file, the frequency domain, phasefreqdet.snf0 file, and the noise results, phasefreqdet.snpn0 file in CosmosScope: 1. Enter cscope at the prompt to start CosmosScope. 2. The time domain results are used to show the input and output waveforms of the phase frequency detector. Use the File > Open > Plotfiles dialog to open the phasefreqdet.sn0 file. Remember to set the file type filter to HSPICE RF. 3. From the signal manager, double-click on the input signals, v(cfin) and v(fin), and the output signals, v(pu) and v(pdn). Figure 5 shows the waveforms for the selected input and output signals. Figure 5 48 Phase Frequency Detector Signals HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator 4. The frequency domain results are used to show the gain of the phase frequency detector. Use the File > Open > Plotfiles dialog to open the phasefreqdet.snf0 file. 5. Open a new XY graph by clicking the waveform icon on the left side of the icon bar. 6. From the signal manager, double-click on the signal v(lfin):(0). The signal is the DC component of the v(lfin) signal spectrum. Both the magnitude and phase of the load current are plotted. To measure the gain of the phase frequency detector verses phase, only the magnitude is required. 7. The Y-axis should be a real value, not a dB value. To change the Y-axis, right-click on the Y-axis and select Attributes from the menu. In the Signal Attributes window, change the view from db(y) to real(y). Figure 6 shows the gain of the phase frequency detector. Figure 6 Phase Frequency Detector Gain 8. Next, plot the output noise of the phase frequency detector. Use the File > Open > Plotfiles dialog to open the phasefreqdet.snpn0 file. 9. Open a new XY graph by clicking the waveform icon on the left side of the icon bar. 10. From the signal manager, double-click on the signal inoise(onoise())). The noise results are shown in Figure 7 on page 50. This displays the noise at the output, v(lfin) at each phase value swept in the .SN command. HSPICE® RF User Guide Z-2007.03 49 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator 11. Change the X-axis scale to log by right-clicking on the X-axis and selecting scale -> log. You can change the color of each trace and control the labeling by right-clicking on the signal name and selecting Member Attributes from the menu. To assign each trace a different color, click on the rainbowcolored button in the Member Attributes menu. The labels are enabled by clicking Show All Labels. Figure 7 Phase Detector Output Noise Ring Oscillator Example The Shooting Newton algorithm provides fast and effective analysis for ring oscillators. The ringoscSN.sp input file for this example is located in the following directory: $installdir/demo/hspicerf/examples/ The analysis finds the oscillation frequency of the ring oscillator. Since the circuit is an oscillator, no input source is required. The oscillator is started by setting an initial condition at the input of the ring (node 1). In the .SNOSC command, the node that the analysis will probe for oscillation conditions is specified, as well as the approximate frequency of oscillation. The number of harmonics to include in the analysis is specified, as well. 50 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator The phase noise characteristics of the oscillator are analyzed by using the .PHASENOISE command. The .PHASENOISE command requires that an output node, pair of nodes, or a two-port element and a frequency sweep be specified. The frequency sweep is used to calculate the phase noise analysis at the specified offset frequencies, measured from the oscillation carrier frequency. For this example phase noise analysis, the default Nonlinear Perturbation (NLP) method is used. The signals v(7) will be probed in both the frequency and time domain. The measure statement is used to measure the fundamental frequency of the oscillator. Simulation Status Output During the simulation, the simulation status is displayed on the screen. In addition to the screen display, more detailed status, cpu time and memory usage information is also written to the ringoscSN.lis file. Parsing Loading Netlist Data Checking Compressing Simulation Time Domain RF Analysis Steady-State Time Domain Analysis will use the matrix-implicit gmres solver. Input period: 2.98507e-09 Starting Shooting Newton Analysis begin circuit stabilization time 20% ... 40% ... 60% ... 80% ... 100% stabilization time done initial frequency: 3.33854e+08 computed period: 2.99532e-09 ***************************************************** ********** Shooting-Newton iteration 1 ************** ***************************************************** 20% 40% 60% 80% HSPICE® RF User Guide Z-2007.03 51 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator 100% number of transient points: 162 start GMRES number of GMRES iterations: 4 updated period: 2.98848e-09 current residual: 6.79374e-09 voltage residual: 0.000183225 : : ***************************************************** ********** Shooting-Newton iteration 5 ************** ***************************************************** 20% ... 40% ... 60% ... 80% ... 100% number of transient points: 2911 start GMRES number of GMRES iterations: 4 updated period 2.98403e-09 current residual: 3.20824e-11 voltage residual: 3.42679e-10 period relative error: 6.7151e-12 value of oscillation frequency found: 3.351176768144e+08 20% ... 40% ... 60% ... 80% ... 100% Finished Shooting Newton Analysis Steady-State Time Domain has converged successfully in 5 iterations DC operating point time = 0 cpu seconds. Shooting-Newton time = 26.04 cpu sec Total Shooting-Newton memory = 11.16 Mbytes Viewing Results in CosmosScope You can view the time-domain, ringoscSN.sn0 file, the frequency domain, ringoscSN.snf0 file, and the phase noise, ringoscSN.snpn0 file in CosmosScope. 1. Enter cscope at the prompt to start CosmosScope. 52 HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator 2. Use the File > Open > Plotfiles dialog to open the ringoscSN.sn0 file. Remember to set the file type filter to HSPICE RF. 3. From the signal manager, double-click on the signal v(7). This is the time domain trace shown at the top of Figure 8. 4. Use the File>Open>Plotfiles dialog to open the ringoscSN.snf0 file. 5. From the signal manager, double-click on the signals v(7). This is the frequency domain spectrum shown at the bottom of Figure 8. Figure 8 Ring Oscillator Output 6. To view the phase noise of the ring oscillator, use the File > Open > Plotfiles dialog to open the ringoscSN.snpn0 file. 7. Open a new XY graph by clicking the waveform icon on the left side of the icon bar. 8. From the signal manager, double-click on the signal nlp_l(f). The noise results are shown in Figure 8. Figure 9 on page 54 shows the resulting phase noise results for the oscillator. HSPICE® RF User Guide Z-2007.03 53 Chapter 3: HSPICE RF Tutorial Example 7: Using Shooting Newton Analysis on a Driven Phase Frequency Circuit and a Ring Oscillator Figure 9 Ring Oscillator Phase Noise Other Shooting Newton Analyses The following Shooting Newton Analyses are also supported by HSPICE RF but not used in this tutorial. 54 ■ .SNFT is equivalent to the .FFT command in transient (.TRAN) analysis. .SNFT uses Fourier transform to represent a time domain signal in the frequency domain. For more information, see Shooting Newton with Fourier Transform (.SNFT). ■ .SNAC is used to perform a linear analysis of a driven (or nonautonomous) circuit, where the linear coefficients are modulated by a periodic, steadystate signal. The functionality is similar to the .HBAC command. For more information, see Shooting Newton AC Analysis (.SNAC). ■ .SNXF is used to calculate transfer functions from an arbitrary number of small signal sources to a designated output in a circuit under periodic steady state conditions. For more information, see Shooting Newton Transfer Function Analysis (.SNXF). HSPICE® RF User Guide Z-2007.03 Chapter 3: HSPICE RF Tutorial Demonstration Input Files Demonstration Input Files The following is a listing of shipped demonstration files for illustrating HSPICE RF functionality. All of these example files are available at: $<installdir>/demo/hspicerf/examples File Name Description acpr.sp Envelope simulation example bjt.inc Transistor model library used by osc.sp mos49_model.inc Transistor model library used by example circuits gpsvco.sp Oscillator and Phase Noise analysis example gsmlna.sp LNA Linear analysis example mix_hb.sp Mixer HB analysis example mix_hbac.sp MIxer HBAC analysis example mix_tran.sp Mixer transient analysis example osc.sp Oscillator tuning curve and phase noise analysis example pa.sp Power amplifier HB analysis example gsmlnaIP3.sp 3rd order intercept point example ringoscSN.sp Shooting Newton and Phase Noise analysis example phasefreqdet.sp Shooting Newton and noise analysis example tsmc018.m Transistor model library used by ringoscSN.sp cmos90nmWflicker.lib Transistor model library used by phasefreqdet.sp HSPICE® RF User Guide Z-2007.03 55 Chapter 3: HSPICE RF Tutorial Demonstration Input Files 56 HSPICE® RF User Guide Z-2007.03 4 4 Input Netlist and Data Entry Describes the input netlist file and methods of entering data. For descriptions of individual HSPICE commands referenced in this chapter, see Chapter 3, RF Netlist Commands, in the HSPICE and RF Command Reference. Input Netlist File Guidelines HSPICE RF operates on an input netlist file, and store results in either an output listing file or a graph data file. An input file, with the name <design>.sp, contains the following: ■ Design netlist (subcircuits, macros, power supplies, and so on). ■ Statement naming the library to use (optional). ■ Specifies the type of analysis to run (optional). ■ Specifies the type of output desired (optional). An input filename can be up to 1024 characters long. The input netlist file cannot be in a packed or compressed format. To generate input netlist and library input files, HSPICE or HSPICE RF uses either a schematic netlister or a text editor. Statements in the input netlist file can be in any order, except that the first line is a title line, and the last .ALTER submodule must appear at the end of the file and before the .END statement. Note: If you do not place an .END statement at the end of the input netlist file, HSPICE RF issues an error message. HSPICE® RF User Guide Z-2007.03 57 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Netlist input processing is case insensitive, except for file names and their paths. HSPICE RF does 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 not use a character string as a parameter value in HSPICE RF. See Delimiters on page 64. ■ An input statement, or equation can be up to 1024 characters long. ■ 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 single whitespace followed by a backslash ( \) or a double backslash ( \\) at the end of the line that you want to continue. • ■ A single backslash preserves white space. Names must begin with an alphabetic character, but thereafter can contain numbers and the following characters: ! # $ % * + / < > [ ] _ { } : ; ? | . 58 • When you use an asterisk (*) or a question mark (?) with a .PRINT, .PROBE, .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 76. • When you use curly brackets ( { } ), HSPICE converts them to square brackets ( [ ] ) automatically. HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines • Names are input tokens. Token delimiters must precede and follow names. See “Delimiters” below. • Names can be up to 1024 characters long and are not case-sensitive. • Do not use any of the time keywords as a parameter name or node name in your netlist. • The following symbols are reserved operator keywords: , () = “ ‘ Do not use these symbols as part of any parameter or node name that you define. Using any of these reserved operator keywords as names causes a syntax error, and HSPICE RF stops immediately. Special Characters The following table lists the special characters that can be used as part of node names, element parameter names, and element instance names. For detailed discussion, see the appropriate sections in this chapter. Note: To avoid unexpected results or error messages, do not use these mathematical characters * - + ^ and / in a parameter name in HSPICE. Table 4 HSPICE/ HSPICE RF Netlists, Net Name Special Characters Special Character Node Name Note: ✓= character is legal anywhere in the string, first or included Instance Name (cannot be the first character; element key letter only) Parameter Name Delimiters (cannot be the first character, element key letter only) ~ tilde Included only HSPICE ✓, Included only for HSPICE RF Included only n/a ! exclamation point ✓ Included only Included only n/a @ at sign Included only ✓ Included only n/a # pound sign ✓ Included only Included only n/a HSPICE® RF User Guide Z-2007.03 59 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Table 4 HSPICE/ HSPICE RF Netlists, Net Name Special Characters Special Character Node Name Note: ✓= character is legal anywhere in the string, first or included Instance Name (cannot be the first character; element key letter only) Parameter Name Delimiters (cannot be the first character, element key letter only) $ dollar sign Included only Included only (avoid if after a number in node name) Included only % percent Included only HSPICE ✓, Included only for HSPICE RF HSPICE: included n/a only, Illegal in HSPICE RF ^ caret Included only & ampersand Included only HSPICE ✓, Included only for HSPICE RF Included only n/a * asterisk HSPICE: Included only included only (avoid using * in node names), Illegal for HSPICE RF HSPICE: included only (avoid using in parameter names), Illegal in HSPICE RF Comment in both HSPICE/HSPICE RF. Wildcard character. Double asterisk (**) is “To the power of”. ( ) parentheses Illegal Illegal Token delimiter - minus HSPICE: Included only included only HSPICE RF ✓ Included only (avoid usage) n/a _ underscore ✓ Included only Included only n/a 60 In-line comment character HSPICE: included “To the power of”, HSPICE ✓, only (avoid usage), i.e., 2^5, two Included only Illegal in HSPICE raised to the fifth for HSPICE RF RF power Illegal HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Table 4 HSPICE/ HSPICE RF Netlists, Net Name Special Characters Special Character Node Name Note: ✓= character is legal anywhere in the string, first or included Instance Name (cannot be the first character; element key letter only) Parameter Name Delimiters (cannot be the first character, element key letter only) + plus sign HSPICE: Included only included only HSPICE RF ✓ HSPICE: included only (avoid usage); Illegal in HSPICE RF Continues previous line. Except for quoted strings (expressions, paths, algebraics) = equals Illegal Illegal Token delimiter Included only n/a Wildcard in character in both HSPICE and HSPICE RF < Illegal > less/more than HSPICE ✓, Included only included only for HSPICE RF question mark HSPICE ✓, Illegal for HSPICE RF Included only Included only forward slash ✓ Included only HSPICE, included n/a only, (avoid usage) Illegal in HSPICE RF { } curly braces HSPICE: Included only included only, converts { } to [ ] No conversion for HSPICE RF Included only Auto-converts to square brackets ([]) [ ] square brackets Include only Included only n/a ? / HSPICE® RF User Guide Z-2007.03 Included only 61 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Table 4 HSPICE/ HSPICE RF Netlists, Net Name Special Characters Special Character Node Name Note: ✓= character is legal anywhere in the string, first or included Instance Name (cannot be the first character; element key letter only) Parameter Name Delimiters (cannot be the first character, element key letter only) \ backslash (requires a whitespace before to use as a continuation) HSPICE: Included only included only, HSPICE RF ✓ Illegal in HSPICE, Continuation Included only in character for HSPICE RF quoted strings (preserves whitespace) \\ double backslash (requires a whitespace before to use as a continuation) HSPICE: Illegal included only, HSPICE RF ✓ Continuation character for quoted strings Illegal | pipe Included only HSPICE ✓, Include only for HSPICE RF Included only n/a , comma Illegal Illegal Illegal Token delimiter. period Illegal Included only Included only Netlist keyword, (i.e., .TRAN, .DC, etc.). Hierarchy delimiter when used in node names colon Included only Included only Included only Delimiter for element attributes ; semi-colon Included only Included only Included only n/a " " double-quotes Illegal Illegal Illegal Expression and filename delimiter. . : 62 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Table 4 HSPICE/ HSPICE RF Netlists, Net Name Special Characters Special Character Node Name Instance Name (cannot be the first character; element key letter only) Parameter Name Delimiters (cannot be the first character, element key letter only) single quotes Illegal Illegal Expression and Illegal filename delimiter. Blank (whitespace) Use before \ or \\ line continuations Note: ✓= character is legal anywhere in the string, first or included ‘ ’ Tab Token delimiter Tab Token delimiter First Character The first character in every line specifies how HSPICE RF interprets the remaining line. Table 5 lists and describes the valid characters. Table 5 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, HSPICE® RF User Guide Z-2007.03 .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) Comment line (HSPICE) + (plus) Continues previous line 63 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Delimiters ■ An input token is any item in the input file that HSPICE RF recognizes. Input token delimiters are: tab, blank, comma (,), equal sign (=), and parentheses ( ). ■ Single (‘) or double quotes (“) delimit expressions and filenames. ■ Colons (:) delimit element attributes (for example, M1:VGS). ■ Periods (.) indicate hierarchy. For example, X1.X2.n1 is the n1 node on the X2 subcircuit of the X1 circuit. Node Identifiers Node identifiers can be up to 1024 characters long, including periods and extensions. Node identifiers are used for node numbers and node names. ■ Node numbers are valid in the range of 0 through 9999999999999999 (1-1e16). ■ Leading zeros in node numbers are ignored. ■ Trailing characters in node numbers are ignored. For example, node 1A is the same as node 1. ■ While node names can contain any of the following special characters— !#%*/<>_?|.&~ —there are restrictions on their use as a first character. See Node Naming Conventions on page 75 for restrictions. For additional information, see Node Naming Conventions on page 75. ■ 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 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 6), except in subcircuits where instance names begin with X. (Subcircuits 64 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines are sometimes called macros or modules.) Instance names can be up to 1024 characters long. Table 6 Element Identifiers Letter (First Char) Element Example Line C Capacitor Cbypass 1 0 10pf D Diode D7 3 9 D1 E Voltage-controlled voltage source Ea 1 2 3 4 K F Current-controlled current source Fsub n1 n2 vin 2.0 G Voltage-controlled current source G12 4 0 3 0 10 H Current-controlled voltage source H3 4 5 Vout 2.0 I Current source IA 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 S-parameter element S1 nd1 nd2 s_model2 V Voltage source V1 8 0 5 W Transmission Line W1 in1 0 out1 0 N=1 L=1 T ““ U ““ HSPICE® RF User Guide Z-2007.03 65 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Table 6 Element Identifiers (Continued) Letter (First Char) Element Example Line X Subcircuit call X1 2 4 17 31 MULTI WN=100 LN=5 Hierarchy Paths ■ A period (.) indicates path hierarchy. ■ Paths can be up to 1024 characters long. ■ Path numbers compress the hierarchy for post-processing and listing files. ■ The .OPTION PATHNUM controls whether the list files show full path names or path numbers. Numbers You can enter numbers as integer, floating point, floating point with an integer exponent, or integer or floating point with one of the scale factors listed in Table 7. Table 7 66 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 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines Table 7 Scale Factors (Continued) Scale Factor Prefix Symbol Multiplying Factor P pico p 1e-12 F femto f 1e-15 A atto a 1e-18 Note: Scale factor A is not a scale factor in a character string that contains amps. For example, HSPICE interprets the 20amps string as 20e-18mps (20-18amps), but it correctly interprets 20amps as 20 amperes of current, not as 20e-18mps (20-18amps). ■ 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 RF use HSPICE name syntax rules, except that names must begin with an alphabetic character. The other characters must be either a number, or one of these characters: ! # $ % [ ] _ ■ To define parameter hierarchy overrides and defaults, use the .OPTION PARHIER=global | local statement. HSPICE® RF User Guide Z-2007.03 67 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines ■ If you create multiple definitions for the same parameter or option, 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 RF does not warn you when you redefine a parameter. ■ You must define a parameter before you use that parameter to define another parameter. ■ When you select design parameter names, be careful to avoid conflicts with parameterized libraries. ■ To delimit expressions, use single or double quotes. ■ Expressions cannot exceed 1024 characters. ■ For improved readability, use a double slash (\\) at end of a line, to continue the line. ■ You can nest functions up to three levels. ■ Any function that you define can contain up to two arguments. ■ Use the PAR (expression or parameter) function to evaluate expressions in output statements. Input Netlist File Structure An input netlist file should consist of one main program and can contain one or more optional submodules. HSPICE RF uses 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,and .LIB) to structure 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. You must enclose the names of included or internally-specified files in single or double quotation when they begin with a number (0-9). Schematic Netlists HSPICE RF typically use netlisters to generate circuits from schematics, and accept either hierarchical or flat netlists. 68 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Guidelines The process of creating a schematic involves: ■ Symbol creation with a symbol editor. ■ Circuit encapsulation. ■ Property creation. ■ Symbol placement. ■ Symbol property definition. ■ Wire routing and definition Table 8 Input Netlist File Sections Sections Examples Definition Title .TITLE The first line in the netlist is the title of the input netlist file (optional in HSPICE RF). 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, .PROBE, .MEASURE Statements to output variables. Statement to evaluate and report userdefined functions of a circuit. Library, Model and File Inclusion .INCLUDE General include files. .MODEL Element model descriptions. HSPICE® RF User Guide Z-2007.03 69 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition Table 8 Sections End of netlist Input Netlist File Sections (Continued) Examples Definition .LIB Library. .END Required statement; end of netlist. Input Netlist File Composition The HSPICE RF circuit description syntax is compatible with the SPICE input netlist format. Figure 10 shows the basic structure of an input netlist. Figure 10 Basic Netlist Structure Title line: First line is automatically a comment * Comments (all lines beginning with an asterisk) * Input control statements Netlist body: description of circuit topology. .MODEL statements * .OPTION statements .OPTION with option statements .PRINT and other output statements. Analysis statement (such as .POWER, .TRAN) .END Element and input control statements Analysis/output control statements The following is an example of a simple netlist file, called inv_ckt.in. It shows a small inverter test case that measures the timing behavior of the inverter. To create the circuit: 1. Define the MOSFET models for the PMOS and NMOS transistors of the inverter. 2. Insert the power supplies for both VDD and GND power rails. Insert the pulse source to the inverter input. This circuit uses transient analysis and produces output graphical waveform data for the input and output ports of the inverter circuit. 70 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition * 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 descriptions of individual HSPICE commands referenced in netlists, see Chapter 3, RF Netlist Commands, in the HSPICE and RF Command Reference. Title of Simulation You set the simulation title in the first line of the input file. HSPICE or HSPICE RF always reads this line, and uses it as the title of the simulation, regardless of the line’s contents. The simulation prints the title verbatim, in each section heading of the output listing file. To set the title, you can place a .TITLE statement on the first line of the netlist. However, HSPICE or HSPICE RF does not require the .TITLE syntax. The first line of the input file is always the implicit title. If any statement appears as the first line in a file, simulation interprets it as a title, and does not execute it. An .ALTER statement does not support use the .TITLE statement. To change a title for a .ALTER statement, place the title content in the .ALTER statement itself. Comments and Line Continuation The first line of a netlist is always a comment, regardless of its first character; comments that are not the first line of the netlist require an asterisk (*) as the HSPICE® RF User Guide Z-2007.03 71 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition first character in a 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 either: ■ Whitespace ■ Comma (,) ■ Valid numeric expression. You can also place the dollar sign within node or element names. For example, * RF=1K GAIN SHOULD BE 100 $ MAY THE FORCE BE WITH MY CIRCUIT VIN 1 0 PL 0 0 5V 5NS $ 10v 50ns R12 1 0 1MEG $ FEED BACK .PARAM a=1w$comment a=1, w treated as a space and ignored .PARAM a=1k$comment a=1e3, k is a scale factor A dollar sign is the preferred way to indicate comments, because of the flexibility of its placement within the code. Line continuations require a plus sign (+) as the first character in the line that follows. Here is an example of comments and line continuation in a netlist file: .ABC Title Line (HSPICE or HSPICE RF ignores the netlist keyword * on this line, because the first line is always a comment) * This is a comment line .MODEL n1 NMOS $ this is an example of an inline comment * This is a comment line and the following line is a continuation + LEVEL=3 Element and Source Statements Element statements describe the netlists of devices and sources. Use nodes to connect elements to one another. Nodes can be either numbers or names. Element statements specify: 72 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition ■ 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 9 lists the parameters of an element statements. Table 9 Element Parameters Parameter Description elname Element name that cannot exceed 1023 characters, and must begin with a specific letter for each element type: 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 S-parameter model T, U, W Transmission line V Voltage source X Subcircuit call node1 ... Node names identify the nodes that connect to the element. The node name begins with a letter and can contain a maximum of 1023 characters. You cannot use the following characters in node names:=( ),’ <space> mname HSPICE or HSPICE RF requires a model reference name for all elements, except passive devices. pname1 ... An element parameter name identifies the parameter value that follows this name. expression Any mathematical expression containing values or parameters, such as param1 * val2 HSPICE® RF User Guide Z-2007.03 73 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition Table 9 Element Parameters (Continued) Parameter Description 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. Example 2 M1 ADDR SIG1 GND SBS N1 w1+w l1+l The preceding example specifies a MOSFET named M1, where: 74 ■ drain node=ADDR ■ gate node=SIG1 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition ■ 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. You can use either names or numbers to designate nodes. Node numbers can be from 1 to 999999999999999; node number 0 is always ground. HSPICE or HSPICE RF ignores letters that follow numbers in node names. When the node name begins with a letter or a valid special character, the node name can contain a maximum of 1024 characters. In addition to letters and digits, node names can include, but NOT begin with the following special characters: +, -, *, /, $, #, [], !, <>, _, %, ~ Node names that begin with one or more numerical digits cannot contain brackets; for example, 123[r55]. Whereas, node names that begin with alphabetic character may contain brackets; for example, n123[r55]. HSPICE® RF User Guide Z-2007.03 75 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition If you use braces { } in node names, HSPICE or HSPICE RF changes them to brackets [ ]. You cannot use the following characters in node names: () ,=‘ <blank> You should avoid using the dollar sign ($) after a numerical digit in a node name, because HSPICE assumes whatever follows the “$” symbol is an in-line comment (see Comments and Line Continuation on page 71 for additional information). It can cause error and warning messages depending on where the node containing the “$” is located. For example, HSPICE generates an error indicating that a resistor node is missing: R1 1$ 2 1k Also, in this example, HSPICE issues a warning indicating that the value of resistor R1 is limited to 1e-5 and interprets the line as “R1 2 1“without a defined value: R1 2 1$ 1k The period (.) is reserved for use as a separator between a subcircuit name and a node name: subcircuitName.nodeName. If a node name contains a period, the node will be considered a top level node unless there is a valid match to a subcircuit name and node name in the hierarchy. The sorting order for operating point nodes is: a-z, !, #, $, %, *, +, -, / Using Wildcards on Node Names You can use wildcards to match node names. ■ ? wildcard matches any single character. For example, 9? matches 92, 9a, 9A, and 9%. ■ * wildcard matches any string of zero or more characters. For example: • 76 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). HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition • ■ 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) Wildcards must begin with a letter or a number; for example, .PROBE v(*) .PROBE * .PROBE x* $ correct format $ incorrect format $ correct format Here are some practical applications for these wildcards: ■ If your netlist includes a resistor named r1 and a voltage source named vin, then .PRINT i(*) prints the current for both elements i(r1) and i(vin). ■ The statement .PRINT v(o*) prints the voltages for all nodes whose names start with o; if your netlist contains nodes named in and out, this example prints only the v(out) voltage. ■ If your netlist contains nodes named 0, 1, 2, and 3, then .PRINT v(0,*) or .PRINT v(0 *) prints the voltage between node 0 and each of the other nodes: v(0,1), v(0,2), and v(0,3). Examples The following examples use wildcards with .PRINT, .PROBE, and .LPRINT statements. ■ Probe node voltages for nodes at all levels. .PROBE v(*) ■ Probe all nodes whose names start with “a”. For example: a1, a2, a3, a00, ayz. HSPICE® RF User Guide Z-2007.03 77 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition .PROBE v(a*) ■ Print node voltages for nodes at the first level and all levels below the first level, where zero-level are top-level nodes. For example: X1.A, X4.554, Xab.abc123. .PRINT v(*.*) ■ Probe node voltages for all nodes whose name start with “x” at the first level and all levels below the first level, where zero-level are top-level nodes. For example: x1.A, x4.554, xab.abc123. .PROBE v(x*.*) ■ Print node voltages for nodes whose names start with “x” at the second-level and all levels below the second level. For example: x1.x2.a, xab.xdff.in. .PRINT v(x*.*.*) ■ 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 72). 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. 78 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition 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. 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, .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 11 on page 79. Figure 11 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 11, 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) HSPICE® RF User Guide Z-2007.03 79 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition 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 probing current—for example .PROBE I(R1)— HSPICE inserts a zero-valued voltage source. This source inserts an extra node in the circuit named Vnn, where nn is a number that HSPICE (or HSPICE RF) automatically generates; this number appears in the output listing file. Global Node Names The .GLOBAL statement globally assigns a node name, in HSPICE or HSPICE RF. This means that all references to a global node name, used at any level of the hierarchy in the circuit, connect to the same node. 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. 80 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition 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 RF supports .DATA only for: ■ Data-driven analysis. ■ Inline or external data files. 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 RF encounters each .LIB call name in the main data file, it reads the corresponding entry from the designated library file, until it finds an .ENDL statement. You can also place a .LIB call statement in an .ALTER block. Library Building Rules ■ A library cannot contain .ALTER statements. ■ A library can contain nested .LIB calls to itself or to other libraries. If you use a relative path in a nested .LIB call, the path starts from the directory of the parent library, not from the work directory. If the path starts from the work directory, HSPICE can also find the library, but it prints a warning. The depth of nested calls is limited only by the constraints of your system configuration. ■ A library cannot contain a call to a library of its own entry name, within the same library file. HSPICE® RF User Guide Z-2007.03 81 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition ■ A HSPICE RF library cannot contain the .END statement. ■ .ALTER processing cannot change .LIB statements, within a file that an .INCLUDE statement calls. 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 RF provides several specialized analysis types, which require a way to control the analysis. For the syntax used in these .PARAM commands, see the description of the .PARAM command in the HSPICE and HSPICE RF Command Reference. HSPICE RF supports the following predefined analysis parameters: ■ Temperature functions (fn) ■ Optimization guess/range ■ Monte Carlo functions HSPICE RF does not support: ■ frequency ■ time 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. Altering Design Variables and Subcircuits The following rules apply when you use an .ALTER block to alter design variables and subcircuits in HSPICE RF. 82 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition ■ If the name of a new element, .MODEL statement, or subcircuit definition is identical to the name of an original statement of the same type, then the new statement replaces the old. Add new statements in the input netlist file. ■ You can alter element and .MODEL statements within a subcircuit definition. You can also add a new element or .MODEL statement to a subcircuit definition. To modify the topology in subcircuit definitions, put the element into libraries. To add a library, use .LIB; to delete, use .DEL LIB. ■ If a parameter name in a new .PARAM statement in the .ALTER module is identical to a previous parameter name, then the new assigned value replaces the old value. ■ If you used parameter (variable) values for elements (or model parameter values) when you used .ALTER, use the .PARAM statement to change these parameter values. Do not use numerical values to redescribe elements or model parameters. ■ If you used an .OPTION statement (in an original input file or a .ALTER block) to turn on an option, you can turn that option off. ■ Each .ALTER simulation run prints only the actual altered input. A special .ALTER title identifies the run. ■ .ALTER processing cannot revise .LIB statements within a file that an .INCLUDE statement calls. However, .ALTER processing can accept .INCLUDE statements, within a file that a .LIB statement calls. Using Multiple .ALTER Blocks The following is the process for using multiple .ALTER blocks: ■ For the first simulation run, HSPICE RF reads the input file, up to the first .ALTER statement, and performs the analyses up to that .ALTER statement. ■ After it completes the first simulation, HSPICE RF reads the input between the first .ALTER statement, and either the next .ALTER statement or the .END statement. ■ HSPICE RF then uses these statements to modify the input netlist file. ■ HSPICE RF then resimulates the circuit. ■ For each additional .ALTER statement, HSPICE RF performs the simulation that precedes the first .ALTER statement. ■ HSPICE RF then performs another simulation, using the input between the current .ALTER statement, and either the next .ALTER statement or the .END statement. HSPICE® RF User Guide Z-2007.03 83 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition 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. Altering Design Variables and Subcircuits The following rules apply when you use an .ALTER block to alter design variables and subcircuits in HSPICE RF. ■ If the name of a new element, .MODEL statement, or subcircuit definition is identical to the name of an original statement of the same type, then the new statement replaces the old. Add new statements in the input netlist file. ■ You can alter element and .MODEL statements within a subcircuit definition. You can also add a new element or .MODEL statement to a subcircuit definition. To modify the topology in subcircuit definitions, put the element into libraries. To add a library, use .LIB; to delete, use .DEL LIB. ■ If a parameter name in a new .PARAM statement in the .ALTER module is identical to a previous parameter name, then the new assigned value replaces the old value. ■ If you used parameter (variable) values for elements (or model parameter values) when you used .ALTER, use the .PARAM statement to change these parameter values. Do not use numerical values to redescribe elements or model parameters. ■ If you used an .OPTION statement (in an original input file or a .ALTER block) to turn on an option, you can turn that option off. ■ Each .ALTER simulation run prints only the actual altered input. A special .ALTER title identifies the run. ■ .ALTER processing cannot revise .LIB statements within a file that an .INCLUDE statement calls. However, .ALTER processing can accept .INCLUDE statements, within a file that a .LIB statement calls. Using Multiple .ALTER Blocks 84 This section does not apply to HSPICE RF. HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition ■ For the first simulation run, HSPICE reads the input file, up to the first .ALTER statement, and performs the analyses up to that .ALTER statement. ■ After it completes the first simulation, HSPICE reads the input between the first .ALTER statement, and either the next .ALTER statement or the .END statement. ■ HSPICE then uses these statements to modify the input netlist file. ■ HSPICE then resimulates the circuit. ■ For each additional .ALTER statement, HSPICE performs the simulation that precedes the first .ALTER statement. ■ HSPICE then performs another simulation, using the input between the current .ALTER statement, and either the next .ALTER statement or the .END statement. If you do not want to rerun the simulation that precedes the first .ALTER statement, every time you run an .ALTER simulation, then do the following: 1. Put the statements that precede the first .ALTER statement, into a library. 2. Use the .LIB statement in the main input file. 3. Put a .DEL LIB statement in the .ALTER section, to delete that library for the .ALTER simulation run. Connecting Nodes Use a .CONNECT statement to connect two nodes in your HSPICE netlist, so that simulation evaluates two nodes as only one node. Both nodes must be at the same level in the circuit design that you are simulating: you cannot connect nodes that belong to different subcircuits. You also cannot use this statement in HSPICE RF. 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. HSPICE® RF User Guide Z-2007.03 85 Chapter 4: Input Netlist and Data Entry Input Netlist File Composition Ending a Netlist An .END statement must be the last statement in the input netlist file. Text that follows the .END statement is a comment, and has no effect on the simulation. An input file that contains more than one simulation run must include an .END statement for each simulation run. You can concatenate several simulations into a single file. Condition-Controlled Netlists (IF-ELSE) You can use the IF-ELSE structure to change the circuit topology, expand the circuit, set parameter values for each device instance, select different model cards, reference subcircuits, or define subcircuits in each IF-ELSE block. .if (condition1) <statement_block1> # The following statement block in {braces} is # optional, and you can repeat it multiple times: { .elseif (condition2) <statement_block2> } # The following statement block in [brackets] # is optional, and you cannot repeat it: [ .else <statement_block3> ] .endif 86 ■ In an .IF, .ELSEIF, or .ELSE condition statement, complex Boolean expressions must not be ambiguous. For example, change (a==b && c>=d) to ( (a==b) && (c>=d) ). ■ In an IF, ELSEIF, or ELSE statement block, you can include most valid HSPICE or HSPICE RF analysis and output statements. The exceptions are: • .END, .ALTER, .GLOBAL, .DEL LIB, .MALIAS, .ALIAS, .LIST, .NOLIST, and .CONNECT statements. • search, d_ibis, d_imic, d_lv56, biasfi, modsrh, cmiflag, nxx, and brief options. HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Using Subcircuits ■ You can include IF-ELSEIF-ELSE statements in subcircuits and subcircuits in IF-ELSEIF-ELSE statements. ■ You can use IF-ELSEIF-ELSE blocks to select different submodules to structure the netlist (using .INC, .LIB, and .VEC statements). ■ If two or more models in an IF-ELSE block have the same model name and model type, they must also be the same revision level. ■ Parameters in an IF-ELSE block do not affect the parameter value within the condition expression. HSPICE or HSPICE RF updates the parameter value only after it selects the IF-ELSE block. ■ You can nest IF-ELSE blocks. ■ You can include .SUBCKT and .MACRO statements within an IF-ELSE block. ■ You can include an unlimited number of ELSEIF statements within an IF-ELSE block. ■ You cannot 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 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. HSPICE® RF User Guide Z-2007.03 87 Chapter 4: Input Netlist and Data Entry Using Subcircuits Figure 12 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). Hierarchical Parameters You can use two hierarchical parameters, the M (multiply) parameter and the S (scale) parameter. M (Multiply) Parameter The most basic HSPICE RF subcircuit parameter 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. To simulate 32 output buffers switching simultaneously, you need to place only one subcircuit; for example, 88 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Using Subcircuits X1 in out buffer M=32 Figure 13 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 EXPANDED Multiply works hierarchically. For a subcircuit within a subcircuit, HSPICE RF multiplies the product of both levels. Do not assign a negative value or zero as the M value. 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 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. HSPICE® RF User Guide Z-2007.03 89 Chapter 4: Input Netlist and Data Entry Using Subcircuits x1 a y inv S=1u subckt inv in out x2 a b kk S=1m .ends In this example: ■ 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 14 on page 90. 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 Figure 14 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 statements, specify the full subcircuit path and node name. 90 HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry DDL Library Access 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 72 and the HSPICE Elements and Device Models Manual for descriptions of element statements. Optional parameter fields in the element statement can override the internal specification of the model. For example, for op-amp devices, you can override the offset voltage, and the gain and offset current. Because the DDL library devices are based on HSPICE circuit-level models, simulation automatically compensates for the effects of supply voltage, loading, and temperature. HSPICE or HSPICE RF accesses DDL models in several ways: ■ The installation script creates an hspice.ini initialization file. ■ HSPICE or HSPICE RF writes the search path for the DDL and vendor libraries into a .OPTION SEARCH=‘<lib_path>’ statement. This provides immediate access to all libraries for all users. It also automatically includes the models in the input netlist. If the input netlist references a model or subcircuit, HSPICE or HSPICE RF searches the directory to which the DDLPATH environment variable points for a file with the same name as the reference name. This file is an include file so its filename suffix is .inc. HSPICE installation sets the DDLPATH variable in the meta.cfg configuration file. ■ Set .OPTION SEARCH=‘<lib_path>’ in the input netlist. Use this method to list the personal libraries to search. HSPICE 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: HSPICE® RF User Guide Z-2007.03 91 Chapter 4: Input Netlist and Data Entry Vendor Libraries .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. Figure 15 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 ... 92 .macro buffer in out vdd vss m1 out in vdd vdd nch w=10 l=1 ... HSPICE® RF User Guide Z-2007.03 Chapter 4: Input Netlist and Data Entry Subcircuit Library Structure 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® RF User Guide Z-2007.03 93 Chapter 4: Input Netlist and Data Entry Subcircuit Library Structure 94 HSPICE® RF User Guide Z-2007.03 5 5 Parameters and Functions Describes how to use parameters within HSPICE RF netlists. 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 RF commands referenced in this chapter, see Chapter 3, RF Netlist Commands, in the HSPICE and RF Command Reference. Using Parameters in Simulation (.PARAM) Defining Parameters Parameters in HSPICE are names that you associate with numeric values. (See Assigning Parameters on page 97.) You can use any of the methods described in Table 10 to define parameters. Table 10 .PARAM Statement Syntax Parameter Description Simple assignment .PARAM <SimpleParam>=1e-12 HSPICE® RF User Guide Z-2007.03 95 Chapter 5: Parameters and Functions Using Parameters in Simulation (.PARAM) Table 10 .PARAM Statement Syntax (Continued) Parameter Description Algebraic definition .PARAM <AlgebraicParam>=‘SimpleParam*8.2’ SimpleParam excludes the output variable. You can also use algebraic parameters in .PRINT and .PROBE statements. For example: .PRINT AlgebraicParam=par(’algebraic expression’) You can use the same syntax for .PROBE, statements. See Using Algebraic Expressions on page 99. 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 .PARAM <mcVar>=Agauss(1.0,0.1) analysis function .MEASURE statement .MEASURE <DC | AC | TRAN> result TRIG ... + TARG ... <GOAL=val> <MINVAL=val> + <WEIGHT=val> <MeasType> <MeasParam> .PRINT | .PROBE .PRINT | .PROBE + 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. 96 HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Using Parameters in Simulation (.PARAM) All parameter values in HSPICE are IEEE double floating point numbers. The parameter resolution order is: 1. Resolve all literal assignments. 2. Resolve all expressions. 3. Resolve all function calls. Table 11 shows the parameter passing order. Table 11 Parameter Passing Order .OPTION PARHIER=GLOBAL .OPTION PARHIER=LOCAL Analysis sweep parameters Analysis sweep parameters .PARAM statement (library) .SUBCKT call (instance) .SUBCKT call (instance) .SUBCKT definition (symbol) .SUBCKT definition (symbol) .PARAM statement (library) Assigning Parameters You can assign the following types of values to parameters: ■ Constant real number ■ Algebraic expression of real values ■ Predefined function ■ Function that you define ■ Circuit value ■ Model value To invoke the algebraic processor, enclose a complex expression in single quotes. A simple expression consists of one parameter name. The parameter keeps the assigned value, unless: ■ A later definition changes its value, or ■ An algebraic expression assigns a new value during simulation. HSPICE does not warn you, if it reassigns a parameter. HSPICE® RF User Guide Z-2007.03 97 Chapter 5: Parameters and Functions Using Parameters in Simulation (.PARAM) 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, .PROBE or .MEASURE statement, use the PAR keyword. Example .PRINT DC v(3) gain=PAR(‘v(3)/v(2)’) PAR(‘v(4)/v(2)’) User-Defined Function Parameters You can define a function that is similar to the parameter assignment, but you cannot nest the functions more than two deep. ■ An expression can contain parameters that you did not define. ■ A function must have at least one argument, and can have up to 20 (and in many cases, more than 20) arguments. ■ You can redefine functions. The format of a function is: funcname1(arg1[,arg2...])=expression1 + [funcname2(arg1[,arg2...])=expression2] off 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 .PARAM f(a,b)=POW(a,2)+a*b g(d)=SQRT(d) + h(e)=e*f(1,2)-g(3) 98 HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Using Algebraic Expressions Predefined Analysis Function HSPICE includes specialized analysis types, such as Optimization and Monte Carlo, that require a way to control the analysis. Measurement Parameters .MEASURE statements produce a measurement parameter. The rules for measurement parameters are the same as for standard parameters, except that measurement parameters are defined in a .MEASURE statement, not in a .PARAM statement.. .PRINT and .PROBE Parameters .PRINT,and.PROBE 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 or.PROBE statement, not in a .PARAM statement 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 .PRINT, statements. Algebraic expressions can expand your options in an input netlist file. Some uses of algebraic expressions are: ■ Parameters: .PARAM x=’y+3’ HSPICE® RF User Guide Z-2007.03 99 Chapter 5: Parameters and Functions Built-In Functions and Variables ■ Functions: .PARAM rho(leff,weff)=’2+*leff*weff-2u’ ■ Algebra in elements: R1 1 0 r=’ABS(v(1)/i(m1))+10’ ■ Algebra in .MEASURE statements: .MEAS vmax MAX V(1) .MEAS imax MAX I(q2) .MEAS ivmax PARAM=’vmax*imax’ ■ Algebra in output statements: .PRINT conductance=PAR(‘i(m1)/v(22)’) The basic syntax for using algebraic expressions for output is: PAR(‘algebraic expression’) In addition to using quotations, you must define the expression inside the PAR( ) statement for output.The continuation character for quoted parameter strings, in HSPICE, is a double backslash (\\). (Outside of quoted strings, the single backslash (\) is the continuation character.) Built-In Functions and Variables In addition to simple arithmetic operations (+, -, *, /), you can use the built-in functions listed in Table 12 and the variables listed in Table 11 on page 97 in HSPICE expressions. Table 12 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) 100 HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Built-In Functions and Variables Table 12 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 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|) HSPICE® RF User Guide Z-2007.03 101 Chapter 5: Parameters and Functions Built-In Functions and Variables Table 12 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function Class Description 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| def(x) parameter defined control Returns 1 if parameter x is defined. min(x,y) smaller of two args control Returns the numeric minimum of x and y max(x,y) larger of two control args Returns the numeric maximum of x and y val(element) get value 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. lv(<Element>) or lx(<Element>) element templates various Returns various element values during simulation. 102 Returns 0 if parameter x is not defined. HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Built-In Functions and Variables Table 12 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function Class Description v(<Node>), i(<Element>)... circuit output variables various Returns various circuit values during simulation. [cond] ?x : y ternary operator Returns x if cond is not zero. Otherwise, returns y. relational operator (less than) Returns 1 if the left operand is less than the right operand. Otherwise, returns 0. relational operator (less than or equal) Returns 1 if the left operand is less than or equal to the right operand. Otherwise, returns 0. relational operator (greater than) Returns 1 if the left operand is greater than the right operand. Otherwise, returns 0. 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. < <= > >= == .param z=’condition ? x:y’ .para x=y<z (y less than z) .para x=y<=z (y less than or equal to z) .para x=y>z (y greater than z) .para x=y>=z (y greater than or equal to z) .para x=y==z (y equal to z) != inequality Returns 1 if the operands are not equal. Otherwise, returns 0. .para x=y!=z (y not equal to z) && Logical AND HSPICE® RF User Guide Z-2007.03 Returns 1 if neither operand is zero. Otherwise, returns 0. .para x=y&&z (y AND z) 103 Chapter 5: Parameters and Functions Parameter Scoping and Passing Table 12 Synopsys HSPICE Built-in Functions (Continued) HSPICE Form Function || Logical OR Class Description 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 13 on page 104 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 13 Synopsys HSPICE Special Variables HSPICE Form Function Class Description time current simulation time control Uses parameters to define the current simulation time, during transient analysis. 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. 104 HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Parameter Scoping and Passing 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. Library Integrity Integrity is a fundamental requirement for any symbol library. Library integrity can be as simple as a consistent, intuitive name scheme, or as complex as libraries with built-in range checking. Library integrity might be poor if you use libraries from different vendors in a circuit design. Because names of circuit parameters are not standardized between vendors, two components can include the same parameter name for different functions. For example, one vendor might build a library that uses the name Tau as a parameter to control one or more subcircuits in their library. Another vendor might use Tau to control a different aspect of their library. If you set a global parameter named Tau to control one library, you also modify the behavior of the second library, which might not be the intent. If the scope of a higher-level parameter is global to all subcircuits at lower levels of the design hierarchy, higher-level definitions override lower-level parameter values with the same names. The scope of a lower-level parameter is local to the subcircuit where you define the parameter (but global to all subcircuits that HSPICE® RF User Guide Z-2007.03 105 Chapter 5: Parameters and Functions Parameter Scoping and Passing 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. 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 106 HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Parameter Scoping and Passing 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. 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. 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 HSPICE® RF User Guide Z-2007.03 107 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 14 compares the three primary methods for configuring libraries, to achieve required parameter checking for default MOS transistor widths. Table 14 Method Methods for Configuring Libraries Parameter Location Pros Cons Local On a .SUBCKT definition line Protects library from global circuit parameter definitions, unless you override it. Single location for default values. Global At the global level and on .SUBCKT definition lines Works with all 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. Parameter Defaults and Inheritance Use the .OPTION PARHIER parameter to specify scoping rules. Syntax: .OPTION PARHIER=< GLOBAL | LOCAL > The default setting is GLOBAL. Example This example explicitly shows the difference between local and global scoping for using parameters in subcircuits. The input netlist includes the following: HSPICE® RF User Guide Z-2007.03 108 Chapter 5: Parameters and Functions Parameter Scoping and Passing .OPTION parhier=<global | local> .PARAM DefPwid=1u .SUBCKT Inv a y DefPwid=2u DefNwid=1u Mp1 <MosPinList> pMosMod L=1.2u W=DefPwid Mn1 <MosPinList> nMosMod L=1.2u W=DefNwid .ENDS Set the .OPTION PARHIER=parameter scoping option to GLOBAL. The netlist also includes the following input statements: xInv0 a y0 Inv $ override DefPwid default, $ xInv0.Mp1 width=1u xInv1 a y1 Inv DefPwid=5u $ override DefPwid=5u, $ xInv1.Mp1 width=1u .measure tran Wid0 param=’lv2(xInv0.Mp1)’ $ lv2 is the $ template for .measure tran Wid1 param=’lv2(xInv1.Mp1)’ $ the channel $ width $ ‘lv2(xInv1.Mp1)’ .ENDS Simulating this netlist produces the following results in the listing file: wid0=1.0000E-06 wid1=1.0000E-06 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 16 on page 110 shows a flat representation of a hierarchical circuit, which contains three resistors. HSPICE® RF User Guide Z-2007.03 109 Chapter 5: Parameters and Functions Parameter Scoping and Passing Each of the three resistors obtains its simulation time resistance from the Val parameter. The netlist defines the Val parameter in four places, with three different values. Figure 16 + 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 16 produces the results in Table 15, based on how you set .OPTION PARHIER to local/global: Table 15 110 PARHIER=LOCAL vs. PARHIER=GLOBAL Results Element PARHIER=Local PARHIER=Global r1 1.0 1.0 HSPICE® RF User Guide Z-2007.03 Chapter 5: Parameters and Functions Parameter Scoping and Passing Table 15 PARHIER=LOCAL vs. PARHIER=GLOBAL Results (Continued) Element PARHIER=Local PARHIER=Global r2 2.0 1.0 r3 3.0 1.0 Parameter Passing Solutions The checklist below determines whether you will see simulation differences when you use the default scoping rules. These checks are especially important if your netlists contain devices from multiple vendor libraries. ■ 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® RF User Guide Z-2007.03 111 Chapter 5: Parameters and Functions Parameter Scoping and Passing 112 HSPICE® RF User Guide Z-2007.03 6 Testbench Elements 6 Describes the syntax for the basic and specialized elements supported by HSPICE RF for high-frequency analysis and characterization. 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. For signal integrity applications see the HSPICE Signal Integrity User Guide. HSPICE RF also supports several specialized elements for high-frequency analysis and characterization. Passive Elements This section describes the passive elements: resistors, capacitors, and inductors. See Multi-Terminal Linear Elements for discussion of the W-, T-, and S-elements. This section includes: ■ Resistors ■ Linear Resistors ■ Behavioral Resistors ■ Skin Effect Resistors ■ Frequency-Dependent Resistors ■ Capacitors ■ Charge-Based Capacitors HSPICE® RF User Guide Z-2007.03 113 Chapter 6: Testbench Elements Passive Elements ■ Linear Capacitors ■ Frequency-Dependent Capacitors ■ Inductors ■ Mutual Inductors ■ Linear Inductors ■ Frequency-Dependent Inductors ■ Ideal Transformers ■ Coupled Inductor Element ■ Reluctance Format ■ Ideal Transformer Format in HSPICE RF ■ DC Block and Choke Elements Resistors 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’ ... 114 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. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements Parameter Description TC1 First-order temperature coefficient for the resistor. See the Passive Device Models chapter in the HSPICE Elements and Device Models Manual for temperature-dependent relations. TC2 Second-order temperature coefficient for the resistor. SCALE Element scale factor; scales resistance and capacitance by its value. Default=1.0. R= resistance Resistance value at room temperature. This can be: ■ ■ ■ ■ ■ 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 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 HSPICE® RF User Guide Z-2007.03 115 Chapter 6: Testbench Elements Passive Elements model (see the Passive Device Models chapter in the HSPICE Elements and Device Models Manual), the resistance value is optional. The following are some basic examples for HSPICE RF. Example 1 R1 is a resistor whose resistance follows the voltage at node c. R1 1 0 ‘v(c)’ Example 2 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))’ Example 3 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’ R3 takes its value from the RX parameter, and uses the TC1 and TC2 temperature coefficients, which become 0.001 and 0, respectively. Example 4 You can use the HERTZ keyword to form frequency-dependent resistors. HSPICE RF accurately analyzes these in all time-domain and frequencydomain simulations. In this example, R4 has resistance with both DC and skineffect contributions: R4 in out R='100.0 + sqrt(HERTZ)/1000.0' Linear Resistors Rxxx node1 node2 < modelname > < R = > value < TC1=val > + < TC2=val > < W=val > < L=val > < M=val > + < C=val > < DTEMP=val > < SCALE=val > 116 Parameter Description Rxxx Name of a resistor. node1 and node2 Names or numbers of the connecting nodes. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements Parameter Description modelname Name of the resistor model. value Nominal resistance value, in ohms. R Resistance, in ohms, at room temperature. TC1, TC2 Temperature coefficient. W Resistor width. 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. HSPICE® RF User Guide Z-2007.03 117 Chapter 6: Testbench Elements Passive Elements Behavioral Resistors HSPICE RF accepts equation-based resistors and capacitors. You can specify the value of a resistor or capacitor as an arbitrary equation that involves node voltages or variable parameters. Unlike HSPICE, you cannot use parameters to indirectly reference node voltages in HSPICE RF. Rxxx n1 n2 . . . <R=> ‘equation’ . . . Example R1 A B R=‘V(A) + I(VDD)’ 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. Frequency-Dependent Resistors You can specify frequency-dependent resistors using the R=expression 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 Rxxx n+ n- R=expression(with HERTZ) <CONVOLUTION=0|1|2> + <FBASE=value> <FMAX=value>> Parameter CONVOLUTION Description Indicates which method is used. ■ ■ ■ 118 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. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench 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, 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 Capacitors The following general input syntax is for a capacitor. Cxxx node1 node2 < modelname > < C = > capacitance + < TC1 = val > < TC2 = val > <W = val > < L = val > + < DTEMP = val > < M = val > < SCALE = val > < IC = val > Cxxx n1 n2 . . . C=‘equation’ CTYPE=[0|1|2] Polynomial form: HSPICE® RF User Guide Z-2007.03 119 Chapter 6: Testbench Elements Passive Elements 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. 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. node1 and node2 Names or numbers of connecting nodes. 120 capacitance Nominal capacitance value in Farads. modelname Capacitance model name. C Capacitance at room temperature in Farads. TC1, TC2 First-order and second-order temperature coefficient. W Capacitor width in meters. L Capacitor length in meters. M Multiplier to simulate multiple parallel capacitors. DTEMP Temperature difference between element and circuit. SCALE Scaling factor. IC Initial capacitor voltage. equation Capacitance can be a function of any node voltage, and any branch current, but not a function of time, frequency, or temperature. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements 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: ■ ■ ■ 0, if C depends only on its own terminal voltages—that is, a function of V(n1<, n2>). This is consistent with HSPICE. 1, if C depends only on outside voltages or currents. This is consistent with HSPICE. 2, if C depends on both its own terminal and outside voltages (default for HSPICE RF). HSPICE does not use CTYPE=2. 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 Passive Device Models chapter in the HSPICE Elements and Device Models Manual), the capacitance value is optional. If you use an equation to specify capacitance, the CTYPE parameter determines how HSPICE calculates the capacitance charge. The calculation is different, depending on whether the equation uses a self-referential voltage (that is, the voltage across the capacitor, whose capacitance is determined by the equation). To avoid syntax conflicts, if a capacitor model has the same name as a capacitance parameter, HSPICE or HSPICE RF uses the model name. Example 1 In the following example, C1 assumes its capacitance value from the model, not the parameter. .PARAMETER CAPXX=1 C1 1 2 CAPXX .MODEL CAPXX C CAP=1 Example 2 In the following example, the C1 capacitors connect from node 1 to node 2, with a capacitance of 20 picofarads: HSPICE® RF User Guide Z-2007.03 121 Chapter 6: Testbench Elements Passive Elements C1 1 2 20p In this next example, Cshunt refers to three capacitors in parallel, connected from the node output to ground, each with a capacitance of 100 femtofarads. Cshunt output gnd C=100f M=3 The Cload capacitor connects from the driver node to the output node. The capacitance is determined by the voltage on the capcontrol node, times 1E-6. The initial voltage across the capacitor is 0 volts. Cload driver output C=’1u*v(capcontrol)’ CTYPE=1 IC=0v The C99 capacitor connects from the in node to the out node. The capacitance is determined by the polynomial C=c0 + c1*v + c2*v*v, where v is the voltage across the capacitor. C99 in out POLY 2.0 0.5 0.01 Example 1 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 pF capacitor. ■ C1 calls the CBX model, and its capacitance is not constant. ■ CB is a 10 pF capacitor with an initial voltage of 4V across it. ■ CP is a 0.1 pF capacitor. Example 2 V1 1 0 pwl(0n 0v 100n 10v) V2 2 0 pwl(0n 0v 100n 10v) C1 1 0 C='(V(1) + V(2))*1e-12' CTYPE=2 Example 3 (HSPICE RF Only) C2 1 0 C='1 + TIME' $ Time-varying capacitor Charge-Based Capacitors You can also specify capacitors using behavioral equations for charge. 122 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements Syntax Cxxx n1 n2 Q='equation' dQ C = -------, V = V (n1,n2) is equivalent to: dV Cxxx a b Q=’f(V(a,b))’ (x) . In the preceding equations, d ( x ) = df -----------dx Example 1 C1 a b Q = ’sin(V(a,b)) + V(c,d)*V(a,b)’ This example is equivalent to: C1 a b C = ’cos (V(a,b)) + V(c,d)’ Example 2 C3 3 0 Q = ‘TIME+TIME’ $ supported in HPICE RF only Linear Capacitors Cxxx node1 node2 < modelname > < C=> value < TC1=val > + < TC2=val > <W=val > < L=val > < DTEMP=val > + < M=val > < SCALE=val > < IC=val > Parameter Description Cxxx Name of a capacitor. Must begin with C, followed by up to 1023 alphanumeric characters. node1 and node2 Names or numbers of connecting nodes. value Nominal capacitance value, in Farads. modelname Name of the capacitor model. C Capacitance, in Farads, at room temperature. TC1, TC2 Specifies the temperature coefficient. W Capacitor width. L Capacitor length. HSPICE® RF User Guide Z-2007.03 123 Chapter 6: Testbench Elements Passive Elements Parameter Description M Multiplier to simulate multiple parallel capacitors. DTEMP Temperature difference between element and circuit. SCALE Scaling factor. IC Initial capacitor voltage. Frequency-Dependent Capacitors You can specify frequency-dependent capacitors using the C=’equation’ with the HERTZ keyword. The HERTZ keyword represents the operating frequency. In time domain analyses, an expression with the HERTZ keyword behaves differently according to the value assigned to the CONVOLUTION keyword. Syntax Cxxx n1 n2 C=’equation’ <CONVOLUTION=[0|1|2] + <FBASE=val> <FMAX=val>> Parameter Description n1 n2 Names or numbers of connecting nodes. equation Expressed as a function of HERTZ. If CONVOLUTION=1 or 2 and HERTZ is not used in the equation, CONVOLUTION is turned off and the capacitor behaves conventionally. The equation can be a function of temperature, but it does not support variables of node voltage, branch current, or time. If these variables exist in the expression and CONVOLUTION=1 or 2, then only their values at the operating point are considered in calculation. CONVOLUTION Specifies the method used. ■ ■ 124 0 (default): HERTZ=0 in time domain analysis. 1 or 2: performs Inverse Fast Fourier Transformation (IFFT) linear convolution. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements Parameter Description 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 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...> 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. See the Passive Device Models chapter in the HSPICE Elements and Device Models Manual for temperature-dependent relations. HSPICE® RF User Guide Z-2007.03 125 Chapter 6: Testbench Elements Passive Elements Parameter Description 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: ■ ■ ■ ■ ■ M Multiplier, used to simulate parallel inductors. Default=1.0. DTEMP Temperature difference between the element and the circuit, in degrees Celsius. Default=0.0. R Resistance of the inductor, in ohms. Default=0.0. L=‘equation’ Inductance at room temperature, specified as: ■ ■ ■ 126 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 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. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements Parameter Description c0 c1... Coefficients of a polynomial in the current, describing the inductor value. c0 is the magnitude of the 0th order term, c1 is the magnitude of the 1st order term, and so on. NT=turns Number of turns of an inductive magnetic winding. mname Saturable core model name. See the Passive Device Models chapter in the HSPICE Elements and Device Models Manual for model information. In this syntax, the inductance can be either a value (in units of henries), an equation, a polynomial of the current, or a magnetic winding. Required fields are the two nodes, and the inductance or model name. ■ If you specify parameters, the nodes and model name must be first. Other parameters can be in any order. ■ If you specify an inductor model (see the Passive Device Models chapter in the HSPICE Elements and Device Models Manual), the inductance value is optional. Example 1 In the following example, the L1 inductor connects from the coilin node to the coilout node, with an inductance of 100 nanohenries. L1 coilin coilout 100n Example 2 The Lloop inductor connects from node 12 to node 17. Its inductance is 1 microhenry, and its temperature coefficients are 0.001 and 0. Lloop 12 17 L=1u TC1=0.001 TC2=0 Example 3 The Lcoil inductor connects from the input node to ground. Its inductance is determined by the product of the current through the inductor, and 1E-6. Lcoil input gnd L=’1u*i(input)’ LTYPE=0 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 has a specified DC resistance of 10 ohms. L99 in out POLY 4.0 0.35 0.01 R=10 HSPICE® RF User Guide Z-2007.03 127 Chapter 6: Testbench Elements Passive Elements Example 5 The L inductor connects from node 1 to node, as a magnetic winding element, with 10 turns of wire. L 1 2 NT=10 Mutual Inductors General form: Kxxx Lyyy Lzzz <K=coupling | coupling> Mutual core form: Kaaa Lbbb <Lccc ... <Lddd>> mname <MAG=magnetization> 128 Parameter Description Kxxx Mutual inductor element name. Must begin with K, followed by up to 1023 alphanumeric characters. Lyyy Name of the first of two coupled inductors. Lzzz Name of the second of two coupled inductors. K=coupling Coefficient of mutual coupling. K is a unitless number, with magnitude > 0 and < 1. If K is negative, the direction of coupling reverses. This is equivalent to reversing the polarity of either of the coupled inductors. Use the K=coupling syntax when using a parameter value or an equation, and the keyword “k=” can be omitted. Kaaa Saturable core element name. Must begin with K, followed by up to 1023 alphanumeric characters. Lbbb, Lccc, Lddd Names of the windings about the Kaaa core. One winding element is required, and each winding element must use the magnetic winding syntax. All winding elements with the same magnetic core model should be written in one mutual inductor statement in the netlist. mname Saturable core model name. (See the Passive Device Models chapter in the HSPICE Elements and Device Models Manual for more information.) HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements Parameter Description MAG= Initial magnetization of the saturable core. You can set this to +1, 0, or -1, where +/- 1 refer to positive and negative values of the BS model parameter. (See the Passive Device Models chapter in the HSPICE Elements and Device Models Manual for more information.) magnetization In this syntax, coupling is a unitless value, from zero to one, representing the coupling strength. If you use parameter labels, the nodes and model name must be first. Other arguments can be in any order. If you specify an inductor model (see the Passive Device Models chapter in the HSPICE Elements and Device Models Manual), the inductance value is optional. You can determine the coupling coefficient, based on geometric and spatial information. To determine the final coupling inductance, HSPICE or HSPICE RF divides the coupling coefficient by the square-root of the product of the selfinductances. When using the mutual inductor element to calculate the coupling between more than two inductors, HSPICE or HSPICE RF can automatically calculate an approximate second-order coupling. See the third example below for a specific situation. Note: The automatic inductance calculation is an estimation, and is accurate for a subset of geometries. The second-order coupling coefficient is the product of the two first-order coefficients, which is not correct for many geometries. Example 1 The Lin and Lout inductors are coupled, with a coefficient of 0.9. K1 Lin Lout 0.9 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. HSPICE® RF User Guide Z-2007.03 129 Chapter 6: Testbench Elements Passive Elements 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 Linear Inductors Lxxx node1 node2 <L => inductance <TC1=val> <TC2=val> + <M=val> <DTEMP=val> <IC=val> Parameter Description Lxxx Name of an inductor. node1 and node2 Names or numbers of the connecting nodes. inductance Nominal inductance value, in Henries. L Inductance, in Henries, at room temperature. TC1, TC2 Temperature coefficient. M Multiplier for parallel inductors. DTEMP Temperature difference between the element and the circuit. IC Initial inductor current. 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. 130 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements 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. ■ ■ ■ FBASE Specifies the lower bound of the transient analysis frequency. ■ ■ ■ ■ FMAX HSPICE® RF User Guide Z-2007.03 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. For CONVOLUTION=1 mode, HSPICE starts sampling at this frequency. For CONVOLUTION=2 mode, HSPICE uses this value as the base frequency point for Inverse Fourier Transformation. For recursive convolution, the default value is 0Hz. For linear convolution, HSPICE uses the reciprocal of the transient period. Specifies the possible maximum frequency of interest. The default value is the frequency point where the function reaches close enough to infinity value, assuming that the monotonous function is approaching the infinity value and that it is taken at 10THz. 131 Chapter 6: Testbench Elements Passive Elements Example L1 1 2 L='0.5n + 0.5n/(1 + HERTZ/1e8)' CONVOLUTION=1 fbase=10 + fmax=30meg Ideal Transformers You can use the IDEAL keyword with the K element to designate ideal transformer coupling. Syntax Kxxx Ij Lj <k=IDEAL | IDEAL> The IDEAL keyword replaces the coupling factor value. 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. Equation 1 v1 v2 v3 v4 ---------- = ---------- = ---------- = ---------- = ... L1 L2 L3 L4 Equation 2 0 = ( il ⋅ L1 ) + ( i2 ⋅ L2 ) + ( i3 ⋅ L3 ) + ( i4 ⋅ L4 ) + ... HSPICE RF can solve any i or v in terms of L ratios. For two inductors (non-DC values): Equation 3 v1 v2 ---------- = ---------L1 L2 Equation 4 0 = ( il ⋅ Equation 5 v2 = v1 ⋅ Equation 6 i2 = i1 ⋅ L1 ) + ( i2 ⋅ L2 ) L2 -----L1 L1 -----L2 DC is treated as usual—inductors are treated as short circuits. DC ignores mutual coupling. You can couple inductors that use the INFINITY keyword to IDEAL K elements. All inductors involved must have the INFINITY value, and for K=IDEAL, the ratios of all L values is unity. Then, for two L values: v2 = v1 i2 = -i1 132 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench 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 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). HSPICE® RF User Guide Z-2007.03 133 Chapter 6: Testbench Elements Passive Elements ** ** 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 Coupled Inductor Element This section describes the multiport syntax for coupled inductor elements. This syntax extends the existing linear (Lxxx) and mutual (Kxxx) inductor elements. Two syntax configurations are available: ■ a reluctance format that is used by Star-RCXT for inductance extraction ■ an ideal transformer format that can be used to create balanced converter (that is, balun) models in HSPICE RF. Reluctance Format Syntax Reluctance Inline Form Lxxx n1p n1n ... nNp nNn + RELUCTANCE=(r1, c1, val1, r2, c2, val2, ... , rm, cm, valm) + <SHORTALL=yes | no> <IGNORE_COUPLING=yes | no> Reluctance External File Form Lxxx n1p n1n ... nNp nNn RELUCTANCE + FILE=“<filename1>” [FILE="<filename2>" [...]] 134 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements + <SHORTALL=yes | no> <IGNORE_COUPLING=yes | no> Parameter Description Lxxx Name of a reluctor. Must begin with L, followed by up to 1023 alphanumeric characters n1p n1n ... nNp nNn Names of the connecting terminal nodes. The number of terminals must be even. Each pair of ports represents the location of an inductor. RELUCTANCE Keyword to specify reluctance (inverse inductance). r1, c1, val1, r2, c2, val2, ... rm, cm, valm Reluctance matrix data. In general, K will be sparse and only non-zero values in the matrix need be given. Each matrix entry is represented by a triplet (r,c,val). The value r and c are integers referring to a pair of inductors from the list of terminal nodes. If there are 2*N terminal nodes, there will be N inductors, and the r and c values must be in the range [1,N]. The val value is a reluctance value for the (r,c) matrix location, and the unit for reluctance is the inverse Henry (H-1). Only terms along and above the diagonal are specified for the reluctance_matrix. The simulator fills in the lower triangle to ensure symmetry. If you specify lower diagonal terms, the simulator converts that entry to the appropriate upper diagonal term. If multiple entries are supplied for the same (r,c) location, then only the first one is used, and a warning will be issued indicating that some entries are ignored. All diagonal entries of the reluctance matrix must be assigned a positive value. The reluctance matrix should be positive definite. FILE=”<filename1>” For the external file format, the data files should contain three columns of data. Each row should contain an (r,c,val) triplet separated by white space. The r, c, and val values may be expressions surrounded by single quotes. Multiple files may be specified to allow the reluctance data to be spread over several files if necessary. HSPICE® RF User Guide Z-2007.03 135 Chapter 6: Testbench Elements Passive Elements Parameter Description SHORTALL ■ ■ IGNORE_COUPLING ■ ■ SHORTALL=yes, all inductors in this model are converted to short circuits, and all reluctance matrix values are ignored. SHORTALL=no (default), inductors are not converted to short circuits, and reluctance matrix values are not ignored. IGNORE_COUPLING=yes, all off-diagonal terms are ignored (that is, set to zero). IGNORE_COUPLING=no (default), off-diagonal terms are not ignored. Example This example has 9 segments (or ports) with 12 nodes, and can potentially generate a 9x9 reluctance matrix with 81 elements. L_ThreeNets a 1 1 2 2 a_1 b 4 4 5 5 b_1 c 7 7 8 8 c_1 + RELUCTANCE=( + 1 1 103e9 + 1 4 -34.7e9 + 1 7 -9.95e9 + 4 4 114e9 + 4 7 -34.7e9 + 7 7 103e9 + 2 2 103e9 + 2 5 -34.7e9 + 2 8 -9.95e9 + 5 5 114e9 + 5 8 -34.7e9 + 8 8 103e9 + 3 3 103e9 + 3 6 -34.7e9 + 3 9 -9.95e9 + 6 6 114e9 + 6 9 -34.7e9 + 9 9 103e9 ) + SHORTALL = no IGNORE_COUPLING = no Alternatively, the same element could be specified by using: L_ThreeNets a 1 1 2 2 a_1 b 4 4 5 5 b_1 c 7 7 8 8 c_1 RELUCTANCE + FILE="reluctance.dat" SHORTALL = no IGNORE_COUPLING = no Where reluctance.dat contains: 136 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Passive Elements + + + + + + + + + + + + + + + + + + 1 1 1 4 4 7 2 2 2 5 5 8 3 3 3 6 6 9 1 4 7 4 7 7 2 5 8 5 8 8 3 6 9 6 9 9 103e9 -34.7e9 -9.95e9 114e9 -34.7e9 103e9 103e9 -34.7e9 -9.95e9 114e9 -34.7e9 103e9 103e9 -34.7e9 -9.95e9 114e9 -34.7e9 103e9 The following shows the mapping between the port numbers and node pairs: ------------------------------------------------------------------------------------|Ports | 1 | 2 | 3 | 4 | 5 | 6 | 7 | 8 | 9 | |Node pairs | (a,1) | (1,2) |(2,a_1)| (b,4) | (4,5) |(5,b_1)| (c,7) | (7,8) |(8,c_1)| ------------------------------------------------------------------------------------- Ideal Transformer Format in HSPICE RF The ideal transformer format simplifies modeling of baluns. Previously, baluns were modeled using mutual inductors (K elements) with the IDEAL keyword. Multiple L and K elements were needed for a given balun model. The ideal transformer model allows modeling of a balun using a single L element. In the ideal transformer format, no absolute inductance or reluctance values are specified. Instead, the transformer’s coupling characteristics are specified using inductor number-of-turns values. The behavior of the ideal transformer depends on ratios of the inductors’ number of turns. Syntax Lxxx n1p n1n ... nNp nNn TRANSFORMER_NT=(nt1, ... , ntN) Parameter Description Lxxx Inductor element name. Must begin with L, followed by up to 1023 alphanumeric characters. HSPICE® RF User Guide Z-2007.03 137 Chapter 6: Testbench Elements Passive Elements Parameter Description n1p n1n ... nNp nNn Positive and negative terminal node names. The number of terminals must be even. Each pair of reports represents the location of an inductor. TRANSFORMER_NT Number of turns values. These parameters must match the number of inductors. The ideal transformer element obeys the standard ideal transformer equations: ν ν νN ------1- = ------2- = … = ------nt 1 nt 2 nt N i 1 nt 1 + i 2 nt 2 + …+ i N nt N = 0 Example L1 1 0 0 2 3 0 transformer_nt=(1,2,2) DC Block and Choke Elements In HSPICE RF, you can specify an INFINITY value for capacitors and inductors to model ideal DC block and choke elements. The following input syntax is for the DC block (ideal infinite capacitor): Syntax Cxxx node1 node2 <C=> INFINITY <IC=val> HSPICE RF does not support any other capacitor parameters for DC block elements, because HSPICE RF assumes that the infinite capacitor value is independent of temperature and scaling factors. The DC block acts as an open circuit for all DC analyses. HSPICE RF calculates the DC voltage across the circuit’s nodes. In all other (non-DC) analyses, a DC voltage source of this value represents the DC block (that is, HSPICE RF does not then allow dv/dt variations). The following input syntax is for the Choke (ideal infinite inductor): Syntax Lxxx node1 node2 <L=> INFINITY <IC=val> HSPICE RF does not support any other inductor parameters, because HSPICE RF assumes that the infinite inductance value is independent of temperature and scaling factors. The choke acts as a short circuit for all DC analyses. HSPICE RF calculates the DC current through the inductor. In all other (non- 138 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements DC) analyses, a DC current source of this value represents the choke (that is, HSPICE RF does not then allow di/dt variations). Multi-Terminal Linear Elements A multi-terminal linear element such as 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 is voltage between the conductors that is transmitted from one end of the pair to the other end. 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 The following sections discuss: ■ W-element (Distributed Transmission Lines) ■ T-element (Ideal Transmission Lines) ■ Scattering Parameter Data Element W-element (Distributed Transmission Lines) 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) HSPICE® RF User Guide Z-2007.03 139 Chapter 6: Testbench Elements Multi-Terminal Linear Elements • Measured-parameter input • Skin effect. ■ Model 3: Built-in field solver model ■ Model 4: Frequency-dependent tabular model ■ Model 5: S-parameter Model W-element Statement The general syntax for a lossy (W-element) transmission line element is: RLGC file form: Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <RLGCfile=filename> N=val L=val U Model form: Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <Umodel=modelname> N=val L=val Field solver form: Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <FSmodel=modelname> N=val L=val The number of ports on a single transmission line are not limited. You must provide one input and output port, the ground references, a model or file reference, a number of conductors, and a length. S Model form: Wxxx in1 <in2 <...inx>> refin out1 <out2 <...outx>> + refout <Smodel=modelname> <NODEMAP=XiYj...> N=val L=val Table Model form: Wxxx in1 in2 <...inx>> refin out1 <out2 <...outx>> + refout N=val L=val TABLEMODEL=name 140 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). HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements Parameter Description refin Ground reference for input signal outx Signal output node for the xth transmission line (each input port must have a corresponding output port). refout Ground reference for output signal. N Number of conductors (excluding the reference conductor). L Physical length of the transmission line, in units of meters. RLGCfile=filename File name reference for the file containing the RLGC information for the transmission lines (for syntax, see Using the W-element in the HSPICE Signal Integrity Guide). Umodel=modelname U-model lossy transmission-line model reference name. A lossy transmission line model, used to represent the characteristics of the W-element transmission line. FSmodel= modelname Internal field solver model name. References the PETL internal field solver as the source of the transmission-line characteristics (for syntax, see Using the Field Solver Model section in 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, see the HSPICE Signal Integrity Guide). TABLEMODEL Name of the frequency-dependent tabular model. Example 1 The W1 lossy transmission line connects the in node to the out node: HSPICE® RF User Guide Z-2007.03 141 Chapter 6: Testbench Elements Multi-Terminal Linear Elements W1 in gnd out gnd RLGCfile=cable.rlgc N=1 L=5 Where, ■ Both signal references are grounded ■ The RLGC file is named cable.rlgc ■ The transmission line is 5 meters long. Example 2 The Wcable element is a two-conductor lossy transmission line: Wcable in1 in2 gnd out1 out2 gnd Umodel=umod_1 N=2 + L=10 Where, ■ in1 and in2 input nodes connect to the out1 and out2 output node ■ Both signal references are grounded. ■ umod_1 references the U-model. ■ The transmission line is 10 meters long. 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, 142 ■ in1 and in2 input nodes connect to the out1 and out2 output node. ■ Both signal references are grounded. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements ■ 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 17 shows node numbering for the element syntax. Figure 17 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) [v1]2 Signal Conductors . . . Reference conductor 0 [i2]2 [v2]2 . . . . . . [v1]N + _ [i2]1 [v2]1 2.1 2.2 [i2]N 2.N [v2]N + _ 2’ x For additional information about the W-element, see the W-element Modeling of Coupled Transmission Lines chapter in the HSPICE Signal Integrity User Guide. T-element (Ideal Transmission Lines) 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: HSPICE® RF User Guide Z-2007.03 143 Chapter 6: Testbench Elements Multi-Terminal Linear Elements Txxx in refin out refout mname L=val Parameter Description Txxx Lossless transmission line element name. Must begin with T, followed by up to 1023 alphanumeric characters. in Signal input node. refin Ground reference for the input signal. out Signal output node. refout Ground reference for the output signal. Z0 Characteristic impedance of the transmission line. TD Signal delay from a transmission line, in seconds per meter. L Physical length of the transmission line, in units of meters. Default=1. IC=v1,i1,v2,i2 Initial conditions of the transmission line. Specify the voltage on the input port (v1), current into the input port (i1), voltage on the output port (v2), and the current into the output port (i2). F Frequency at which the transmission line has the electrical length specified in NL. NL Normalized electrical length of the transmission line (at the frequency specified in the F parameter), in units of wavelengths per line length. Default=0.25, which is a quarter-wavelength. mname U-model reference name. A lossy transmission line model, representing the characteristics of the lossless transmission line. Only one input and output port is allowed. Example 1 The T1 transmission line connects the in node to the out node: T1 in gnd out gnd Z0=50 TD=5n L=5 144 ■ Both signal references are grounded. ■ Impedance is 50 ohms. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements ■ 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. Example 3 The Tnet1 transmission line connects the driver node to the output node: Tnet1 driver gnd output gnd Umodel1 L=1m ■ Both signal references are grounded. ■ Umodel1 references the U-model. ■ The transmission line is 1 millimeter long. Ideal Transmission Line For the ideal transmission line, voltage and current will propagate without loss along the length of the line (±x direction) with spatial and time-dependence given according to the following equation: v ( x, t ) = Re [ Ae j ( ωt – βx ) + Be j ( ϖt + βx ) ] B j ( ωt + βx ) A j ( ωt – βx ) ----– e v ( x, t ) = Re ----- e Z0 Z0 The A represents the incident voltage, B represents the reflected voltage, Z0 is the characteristic impedance, 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: HSPICE® RF User Guide Z-2007.03 145 Chapter 6: Testbench Elements Multi-Terminal Linear Elements ω 1 υ ρ = --- = ----------β LC At the end of the transmission line ( x = l ), the propagation term βl becomes the following equation: l βl = ω LC ⋅ l = ω----vp This is equivalent to an ideal delay with the following value: l- = T = ----VP LC ⋅ l Where, T : absolute time delay (sec) l : physical length (L) (meters) VP : phase velocity (meters/sec) Using standard distance=velocity*time relationships, the HSPICE T-element parameter values are related to these terms according to: 1V P = f ⋅ λ = --td Where, f: frequency λ: wavelength td : relative time delay (TD) (sec/meter) l l - = l----------⁄ λ- = = ------ = t d ⋅ l = ----------Vp f⋅ λ f LC ⋅ Where, l: physical length (L) (meters) l ⁄ λ: f: normalized length (NL) frequency at NL (F) (Hz) T = TD ⋅ L = NL ------- = L 146 LC ⋅ L HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements HSPICE therefore allows you to specify a transmission line in three different ways: ■ Z0, TD, L ■ Z0, NL, F ■ L L, with ---- and LC values taken from a U model. C Scattering Parameter Data Element A transmission line is a passive element that connects any two conductors at any distance apart. For more information about transmission lines, see Sparameter Modeling Using the S-element in the HSPICE Signal Integrity Guide. Frequency-Dependent Multi-Terminal (S-element) When used with the generic frequency-domain model (.MODEL SP), an S-element is a convenient way to describe the behavior of a multi-terminal network. The S-element describes a linear time-invariant system, and provides a series of data that describe the frequency response of the system. The S-element is particularly useful for high-frequency characterization of distributed passive structures. A common use of the S-element is in microwave circuits, because electronic devices in this frequency domain no longer act as they do in low frequencies. In this case, distributed system parameters must be considered. The S-element uses the following parameters to define a frequency-dependent, multi-terminal network: ■ S (scattering) parameter ■ Y (admittance) parameter Note: All HSPICE and HSPICE RF analyses can use the S-element. The S-parameter is the reflection coefficient of the system, which is measured through ratios of incident and reflected sinusoidal waves. For passive systems, the magnitude of an S parameter varies between zero and one. Because the reflection coefficient is easy to measure in real microwave circuits, the S parameter can be a very useful tool for microwave engineers. HSPICE® RF User Guide Z-2007.03 147 Chapter 6: Testbench Elements Multi-Terminal Linear Elements You can use the S-element with a .MODEL SP, or with data files that describe the frequency response of a network and provide discrete frequency dependent data (Touchstone and CITIfile). You can measure this data directly using network analyzers such as Hewlett-Packard's MDS (Microwave Design System) or HFSS (High Frequency Structure Simulator). HSPICE can also extract the S element from a real circuit system. For a description of the S parameter and SP analyses, see S-parameter Model in the HSPICE Signal Integrity Guide. S-element Syntax The nodes of the S-element must come first. If MNAME is not declared, you must specify the FQMODEL. You can specify all the optional parameters in both the S-element and S model statements, except for MNAME argument. You can enter the optional arguments in any order, and the parameters specified in the element statement have a higher priority. If the number of nodes in the element card is smaller than the number specified in the model card (or external file) by 1, then the reference node is the default. The default reference node is 0 (gnd). Figure 18 Terminal Node Notation . . . . . . [vinc]1 [i]1 [vref]1 . . . N+1 terminal system [vinc]N [i]N [vref]N ndN (+) [v]N nd1 (+) [v]1 (-) ndR (reference node) S Model Syntax .MODEL Smodel_name S 148 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements + + + + + + + + + <N=dimension> [FQMODEL=sp_model_name | TSTONEFILE=filename | CITIFILE=filename] <TYPE=[s | y]> <Zo=[value | vector_value]> <FBASE=base_frequency> <FMAX=maximum_frequency> <HIGHPASS=[0|1|2]> <LOWPASS=[0|1|2]> <PRECFAC=val> <DELAYHANDLE=[1|0|ON|OFF]> <DELAYFREQ=val> <MIXEDMODE=[0|1]> <DATATYPE=data_string> <XLINELENGTH=val> Parameter Specifies Smodel_name Name of the S model. S Specifies that the model type is an S model. N S model dimension, which is the terminal number of the S-element, excluding the reference node. 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 .sp# 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 frequencydependent data. For details, see Using Instruments with ADS by Agilent Technologies (http://www.agilent.com). TYPE One of the following parameter types: ■ ■ ■ HSPICE® RF User Guide Z-2007.03 S (scattering) (default) Y (admittance) Z (impedance) 149 Chapter 6: Testbench Elements Multi-Terminal Linear Elements Parameter Specifies Zo Characteristic impedance value of the reference line (frequencyindependent). 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 to use for transient analysis. This value becomes the base frequency point for Inverse Fast Fourier Transformation (IFFT). ■ ■ If you do not set this value, the base frequency is a reciprocal value of the transient period. If you set a frequency that is smaller than the reciprocal value of the transient, then the transient analysis performs circular convolution, and uses the reciprocal value of FBASE as its base period. FMAX Maximum frequency for transient analysis. Used as the maximum frequency point for Inverse Fast Fourier Transform (IFFT). 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. ■ 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. ■ PRECFAC 150 Preconditioning factor to avoid a singularity in the form of an infinite admittance matrix. See Pre-Conditioning S-parameters on page 154 for more information. The default=0.75. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements Parameter Specifies DELAYHANDLE Delay handler for transmission line type parameters. ■ 1 or ON activates the delay handler. See Group Delay Handler in Time Domain Analysis on page 153. ■ 0 or OFF (default) deactivates the delay handler. You must set the delay handler, if the delay of the model is longer than the base period specified in the FBASE parameter. If you set DELAYHANDLE=OFF but DELAYFQ is not zero, HSPICE simulates the S-element in delay mode. DELAYFREQ Delay frequency for transmission line type parameters, which is the frequency point when HSPICE RF extracts the matrix delay. The default is the FMAX value, which is the maximum frequency used in the transient analysis. If you set DELAYHANDLE to OFF, but DELAYFREQ is not zero, HSPICE still simulates the S element in delay mode. 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: ■ ■ XLINELENGTH X = D to indicate a differential term = C to indicate a common term = S to indicate a single (grounded) term n = the port number The line length of the transmission line system where the S parameters are extracted. This keyword is required only when the S Model is used in a W element. The FQMODEL, TSTONEFILE, and CITIFILE parameters describe the frequency-varying behavior of a network. Only specify one of the parameters in an S model card. If more than one method is declared, only the first one is used and HSPICE issues a warning message. FQMODEL can be set in S element and S model statements, but both statements must refer to the same model name. The S element is capable of reading in two-port noise parameter data from Touchstone data files and then transform the raw data into a form used for noise (and .LIN 2PNOISE) analysis. HSPICE® RF User Guide Z-2007.03 151 Chapter 6: Testbench Elements Multi-Terminal Linear Elements For example, you can represent a two-port system with an S element and then perform a noise analysis (or any other analysis). The S element noise model supports both normal and two-port noise analysis (.NOISE and .LIN NOISECALC=1). Example 1 s1 n1 n2 n3 n_ref mname=smodel .model smodel s n=3 fqmodel=sfqmodel zo=50 fbase=25e6 + fmax=1e9 Example 2 s1 n1 n2 n3 n_ref fqmodel=sfqmodel zo=50 fbase=25e6 fmax=1e9 Examples 1 and 2 return the same result. Example 3 s1 n1 n2 n3 n_ref mname=smodel zo=100 .model smodel s n=3 fqmodel=sfqmodel zo=50 fbase=25e6 + fmax=1e9 In this example, the characteristic impedance of each port is 100 ohms, instead of 50 ohms as defined in smodel, because parameters defined in the S element statement have higher priority than those defined in the S model statement. Example 4 s1 n1 n2 n3 n_ref mname=smodel .model smodel s n=3 fqmodel=sfqmodel zo=50 50 100 In this example, the characteristic impedance of port1 and port2 are 50 ohms, and the characteristic impedance of port3 is 100 ohms. Example 5 s1 n1 n2 n3 n_ref mname=smodel .model smodel s tstonefile=expl.s3p In this example, the name of the tstone file, expl.s3p, reveals that the network has three ports. Example 6 s1 n1 n2 n3 n_ref mname=smodel .model smodel s fqmodel=sfqmodel tstonefile=expl.s3p + citifile=expl.citi0 152 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Multi-Terminal Linear Elements In this example, fqmodel, tstonefile, and citifile are all declared. HSPICE uses only the fqmodel, ignores tstonefile and citifile, and reports warning messages. Example 7 s1 n1 n2 n3 n_ref mname=smodel fqmodel=sfqmodel_1 .model smodel s n=3 fqmodel=sfqmodel_2 In this example, fqmodel is declared in both the S element statement and the S model statement, and they have different fqmodel names. This is not allowed in HSPICE. Example 8 s1 n1 n2 n3 n_ref mname=smodel fqmodel=sfqmodel .model smodel s tstonefile=expl.s3p In this example, fqmodel is already declared in the s1 statement, and tstonefile is declared in the related smodel card. This is a conflict when describing the frequency-varying behavior of the network, which is not allowed in HSPICE. Frequency Table Model The frequency table model (SP model) is a generic model that you can use to describe frequency-varying behavior. Currently, the S-element and the .LIN command use this model. For a description of this model, see section SmallSignal Parameter Data Frequency Table Model (SP Model) in the HSPICE Signal Integrity User Guide. Group Delay Handler in Time Domain Analysis The S element accepts a constant group delay matrix in time-domain analysis. You can also express a weak dependence of the delay matrix on the frequency as a combination of the constant delay matrix and the phase shift value at each frequency point. To activate or deactivate this delay handler, specify the DELAYHANDLE keyword in the S model statement. The delay matrix is a constant matrix, which HSPICE RF extracts using finite difference calculation at selected target frequency points. HSPICE RF obtains the T ω( i, j ) delay matrix component as: HSPICE® RF User Guide Z-2007.03 153 Chapter 6: Testbench Elements Multi-Terminal Linear Elements Equation 7 T ω( i, j) dθ Sij dθ Sij 1 - = ------ ⋅ -----------= ----------df 2π dω ■ f is the target frequency, which you can set using DELAYFREQ. 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: Equation 8 y′ mn ( ω) = y mn ( ω) × e jωT mn The convolution process then uses the following equation to calculate the delay: Equation 9 i k ( t ) = ( y′ k1 ( t ), y′ k2 ( t ), …, y′ kN ( t ) ) × ( v 1 ( t – TK1 ), v 2 ( t – TK2 ), …, v Nt – TKN ) 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: Equation 10 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 keyword in the S model statement. The default pre-conditioning factor is 0.75. 154 HSPICE® RF User Guide Z-2007.03 T Chapter 6: Testbench Elements Port Element Figure 19 Pre-Conditioning S-parameters S S kRref Preconditioning S’ S to Y Y’ -kRref NMA stamp Y’ Y 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. Port Element Syntax Pxxx p n port=portnumber HSPICE® RF User Guide Z-2007.03 155 Chapter 6: Testbench Elements Port Element + + + + + + + + + + $ **** 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. ■ ■ ■ <transient_waveform> 156 phase is in degrees harm and tone are indices corresponding to the tones specified in the .HB statement. Indexing starts at 1 (corresponding to the first harmonic of a tone). modtone and modharm specify sources for multitone simulation. A source specifies a tone and a harmonic, and up to 1 offset tone and harmonic (modtone for tones and modharm for harmonics). The signal is then described as: V(or I) = mag*cos(2*pi* (harm*tone+modharm*modtone)*t + phase) (Transient analysis) Voltage or power source waveform. Any one of waveforms: AM, EXP, PULSE, PWL, SFFM, or SIN. Multiple transient descriptions are not allowed. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Port Element Parameter Description <TRANFORHB=[0|1]> ■ 0 (default): The transient description is ignored if an HB value is given or a DC value is given. If no DC or HB value is given and TRANFORHB=0, then HB analysis treats the source as a DC source, and the DC source value is the time=0 value. ■ 1: HB analysis uses the transient description if its value is VMRF, SIN, PULSE, PWL, or LFSR. If the type is a non-repeating PWL source, then the time=infinity value is used as a DC analysis source value. For example, the following statement is treated as a DC source with value=1 for HB analysis: v1 1 0 PWL (0 0 1n 1 1u 1) + TRANFORHB=1 In contrast, the following statement is a 0V DC source: v1 1 0 PWL (0 0 1n 1 1u 1) + TRANFORHB=0 The following statement is treated as a periodic source with a 1us period that uses PWL values: v1 1 0 PWL (0 0 1n 1 0.999u 1 1u 0) R + TRANFORHB=1 To override the global TRANFORHB option, explicitly set TRANFORHB for a voltage or current source. DCOPEN Switch for open DC connection when DC mag is not set. ■ ■ <z0=val> 0 (default): P element behaves as an impedance termination. 1 : P element is considered an open circuit in DC operating point analysis. DCOPEN=1 is mainly used in .LIN analysis so the P element will not affect the selfbiasing device under test by opening the termination at the operating point. (LIN analysis) System impedance used when converting to a power source, inserted in series with the voltage source. Currently, this only supports real impedance. ■ When power=0, z0 defaults to 0. When power=1, z0 defaults to 50 ohms. You can also enter zo=val. ■ HSPICE® RF User Guide Z-2007.03 157 Chapter 6: Testbench Elements Port Element 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 impedance. Values are in dbms. You can use this parameter for Transient analysis if the power source is either DC or SIN. Example For example, the following port element specifications identify a 2-port network with 50-ohm reference impedances between the “in” and “out” nodes. P1 in gnd port=1 z0=50 P2 out gnd port=2 z0=50 Computing scattering parameters requires z0 reference impedance values. The order of the port parameters (in the P-element) determines the order of the S, Y, and Z parameters. Unlike the .NET command, the .LIN command does not require you to insert additional sources into the circuit. To calculate the requested transfer parameters, HSPICE automatically inserts these sources as needed at the port terminals. You can define an unlimited number of ports. 158 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Active Elements Using the 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 20 shows the block diagram of the mixed mode port element. Figure 20 Mixed Mode Port Element P1 (Port element) n1+ Z0 V+ Z0 Vn2- n1_ref Pl nl+ nl- nl_ref Zo=50 Active Elements This section describes the active 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> HSPICE® RF User Guide Z-2007.03 159 Chapter 6: Testbench Elements Active Elements + <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> 160 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. 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. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Active Elements Parameter Description OFF Sets the initial condition for this element to OFF, in DC analysis. Default=ON. IC=vd Initial voltage, across the diode element. Use this value when you specify the UIC option in the .TRAN statement. The .IC statement overrides this value. M Multiplier, to simulate multiple diodes in parallel. The M setting affects all currents, capacitances, and resistances. Default=1. DTEMP The difference between the element temperature and the circuit temperature, in degrees Celsius. Default=0.0. W Width of the diode, in meters (LEVEL=3 diode model only) L Length of the diode, in meters (LEVEL=3 diode model only) You must specify two nodes and a model name. If you specify other parameters, the nodes and model name must be first and the other parameters can appear in any order. Example 1 The D1 diode, with anode and cathode, connects to nodes 1 and 2. Diode1 specifies the diode model. D1 1 2 diode1 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 HSPICE® RF User Guide Z-2007.03 161 Chapter 6: Testbench Elements Active Elements Bipolar Junction Transistor (BJT) Element Qxxx nc nb ne <ns> mname <area> <OFF> + <IC=vbeval,vceval> <M=val> <DTEMP=val> Qxxx nc nb ne <ns> mname <AREA=area> <AREAB=val> + <AREAC=val> <OFF> <VBE=vbeval> <VCE=vceval> + <M=val> <DTEMP=val> Parameter Description Qxxx BJT element name. Must begin with Q, then up to 1023 alphanumeric characters. nc Collector terminal node name. nb Base terminal node name. ne Emitter terminal node name. ns Substrate terminal node name, which is optional. You can also use the BULK parameter to set this name in the BJT model. mname BJT model name reference. area, AREA=area Emitter area multiplying factor, which affects currents, resistances, and capacitances. Default=1.0. OFF Sets initial condition for this element to OFF, in DC analysis. Default=ON. 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. 162 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. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Active Elements Parameter Description AREAC Collector area multiplying factor, which affects currents, resistances, and capacitances. Default=AREA. The only required fields are the collector, base, and emitter nodes, and the model name. The nodes and model name must precede other fields in the netlist. Example 1 In the Q1 BJT element below: Q1 1 2 3 model_1 ■ The collector connects to node 1. ■ The base connects to node 2. ■ The emitter connects to node 3. ■ model_1 references the BJT model. Example 2 In the following Qopamp1 BJT element: Qopamp1 c1 b3 e2 s 1stagepnp AREA=1.5 AREAB=2.5 AREAC=3.0 ■ 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. HSPICE® RF User Guide Z-2007.03 163 Chapter 6: Testbench Elements Active Elements ■ The emitter connects to the output node. ■ model_npn references the BJT model. ■ The area factor is 0.1. JFETs and MESFETs Jxxx nd ng ns <nb> mname <<<AREA>=area | <W=val> + <L=val>> <OFF> <IC=vdsval,vgsval> <M=val> + <DTEMP=val> Jxxx nd ng ns <nb> mname <<<AREA>=area> | <W=val> + <L=val>> <OFF> <VDS=vdsval> <VGS=vgsval> + <M=val> <DTEMP=val> 164 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. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Active Elements Parameter Description IC=vdsval, vgsval, VDS, VGS Initial internal drain-source voltage (vdsval) and gate-source voltage (vgsval). Use this argument when the .TRAN statement contains UIC. The .IC statement overrides it. M Multiplier to simulate multiple JFETs or MESFETs in parallel. The M setting affects all currents, capacitances, and resistances. Default=1. DTEMP The difference between the element temperature and the circuit temperature, in degrees Celsius. Default=0.0. Only drain, gate, and source nodes, and model name fields are required. Node and model names must precede other fields. Example 1 In the J1 JFET element below: J1 1 2 3 model_1 ■ The drain connects to node 1. ■ The source connects to node 2. ■ The gate connects to node 3. ■ model_1 references the JFET model. Example 2 In the following Jopamp1 JFET element: Jopamp1 d1 g3 s2 b 1stage AREA=100u ■ 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 HSPICE® RF User Guide Z-2007.03 165 Chapter 6: Testbench Elements Active Elements ■ The drain connects to the driver node. ■ The source connects to the in node. ■ The gate connects to the output node. ■ model_jfet references the JFET model. ■ The width is 10 microns. ■ The length is 10 microns. MOSFETs Mxxx nd ng ns <nb> mname <<L=>length> <<W=>width> + <AD=val> AS=val> <PD=val> <PS=val> + <NRD=val> <NRS=val> <RDC=val> <RSC=val> <OFF> + <IC=vds,vgs,vbs> <M=val> <DTEMP=val> + <GEO=val> <DELVTO=val> .OPTION WL Mxxx nd ng ns <nb> mname <width> <length> <other_options...> 166 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, with a maximum value of 0.1m. Default=DEFL. W MOSFET channel width, in meters. This parameter overrides .OPTION DEFW. Default=DEFW. AD Drain diffusion area. Overrides .OPTION DEFAD. Default=DEFAD, if you set the ACM=0 model parameter. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Active Elements Parameter Description AS Source diffusion area. Overrides .OPTION DEFAS. Default=DEFAS, if you set the ACM=0 model parameter. PD Perimeter of drain junction, including channel edge. Overrides .OPTION DEFPD. Default=DEFAD, if you set the ACM=0 or 1 model parameter. Default=0.0, if you set ACM=2 or 3. PS Perimeter of source junction, including channel edge. Overrides .OPTION DEFPS. Default=DEFAS, if you set the ACM=0 or 1 model parameter. Default=0.0, if you set ACM=2 or 3. NRD Number of squares of drain diffusion for resistance calculations. Overrides .OPTION DEFNRD. Default=DEFNRD, if you set ACM=0 or 1 model parameter. Default=0.0, if you set ACM=2 or 3. NRS Number of squares of source diffusion for resistance calculations. Overrides .OPTION DEFNRS. Default=DEFNRS when you set the MOSFET model parameter ACM=0 or 1. Default=0.0, when you set ACM=2 or 3. RDC Additional drain resistance due to contact resistance, in units of ohms. This value overrides the RDC setting in the MOSFET model specification. Default=0.0. RSC Additional source resistance due to contact resistance, in units of ohms. This value overrides the RSC setting in the MOSFET model specification. Default=0.0. OFF Sets initial condition for this element to OFF, in DC analysis. Default=ON. This command does not work for depletion devices. IC=vds, vgs, vbs Initial voltage across external drain and source (vds), gate and source (vgs), and bulk and source terminals (vbs). Use these arguments with .TRAN UIC. .IC statements override these values. 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® RF User Guide Z-2007.03 167 Chapter 6: Testbench 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=4.0 168 ■ The drain connects to the driver node. ■ The gate connects to the in node. ■ The source connects to the output node. ■ bsim3v3 references the MOSFET model. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Steady-State Voltage and Current Sources ■ 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. Steady-State Voltage and Current Sources The I (current source) and V (voltage source) elements include extensions that allow you to use them as sources of steady-state sinusoidal signals for HB and HBAC analyses. When you use a power parameter to specify the available power, you can also use these elements as power sources. For a general description of the I and V elements, see Power Sources in the HSPICE Simulation and Analysis User Guide. I and V Element Syntax Vxxx p n + $ **** Voltage or Power Information ******** + <<dc> mag> <ac <mag <phase>>> <HBAC <mag <phase>>> + <hb <mag <phase <harm <tone <modharm <modtone>>>>>>> + <transient waveform> <TRANFORHB=[1|0]> + $ **** Power Switch ******** + <power=[0 | 1 | W | dbm]> <z0=val> <rdc=val> <rac=val> + <RHBAC=val> <rhb=val> <rtran=val> Ixxx p n + $ **** Current or Power Information ******** + <<dc> mag> <ac <mag <phase>>> <HBAC <mag <phase>>> + <hb <mag <phase <harm <tone <modharm <modtone>>>>>>> + <transient waveform> <TRANFORHB=[1|0]> + $ **** Power Switch ******** + <power=[0 | 1 | W | dbm]> <z0=val> <rdc=val> <rac=val> + <RHBAC=val> <rhb=val> <rtran=val> Parameter Description <<dc> mag> DC voltage or power source value. You don’t need to specify DC explicitly (default=0). <ac <mag <phase>>> AC voltage or power source value. HSPICE® RF User Guide Z-2007.03 169 Chapter 6: Testbench Elements Steady-State Voltage and Current Sources Parameter Description <HBAC <mag <phase>>> (HSPICE RF) HBAC voltage or power source value. <hb <mag <phase <harm (HSPICE RF) HB voltage, current, or power source value. <tone <modharm Multiple HB specifications with different harm, tone, <modtone>>>>>>> modharm, and modtone values are allowed. ■ ■ ■ <transient waveform> 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 multi-tone simulation. A source specifies a tone and a harmonic, and up to 1 offset tone and harmonic (modtone for tones and modharm for harmonics). The signal is then described as: V(or I) = mag*cos(2*pi* (harm*tone+modharm*modtone)*t + phase) (Transient analysis) Any one of waveforms: AM, EXP, PULSE, PWL, SFFM, or SIN. Multiple transient descriptions are not allowed. <power=[0 | 1 | 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 dbm, element treated as a power source in series with the port impedance. Values are in dbms. You can use this parameter for Transient analysis if the power source is either DC or SIN. <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. ■ <rdc=val> 170 (DC analysis) Series resistance (overrides z0). HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Steady-State Voltage and Current Sources Parameter Description <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). <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 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 source value. For example, the following statement is treated as a DC source with value=1 for HB: 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 V/I source. Example 1 This example shows an HB source for a single tone analysis: .hb tones=100MHz harms=7 I1 1 2 dc=1mA hb 3mA 0. 1 1 I1 is a current source with a the following time-domain description: I1=1mA + 3mA*cos(2*pi*1.e8*t) Example 2 This example shows HB sources used for a two-tone analysis: HSPICE® RF User Guide Z-2007.03 171 Chapter 6: Testbench Elements Steady-State HB Sources .hb tones=1.e9 1.1e9 intmodmax=5 Vin lo 0 dc=0. hb 1.5 90 1 1 Vrf rf 0 dc=0. hb 0.2 0 1 2 These sources have the following time-domain descriptions: Vin=1.5*cos(2*pi*1.e9*t - 90*pi/180) V Vrf = 0.2*cos(2*pi*1.1e9*t) V Example 3 The following HB source uses a modtone and modharms: .hb tones=2.e9 1.9e9 harms=5 5 Vm input gnd dc=0.5 hb 0.2 0. 1 1 -1 2 Vm has the following time-domain description: Vm = 0.5 + cos(2*pi*1.e8*t) Example 4 This example uses an HB source specified with a SIN source and HBTRANINIT. .hb tone=1.e8 harms=7 Vt 1 2 SIN(0.1 1.0 2.e8 0. 0. 90) tranforhb=1 Vt is converted to the following HB source: Vt 1 2 dc=0.1 hb 1.0 0.0 2 1 Example 5 This example shows a power source (the units are Watts). .hb tones=1.1e9 harms=9 Pt Input Gnd power=1 Z0=50. 1m 0. 1 1 Pt delivers 1 mW of power through a 50 ohm impedance. Steady-State HB Sources The fundamental frequencies used with harmonic balance analysis are specified with the .HB TONES command. These frequencies can then be referenced by their integer indices when specifying steady-state signal sources. For example, the .HB specification given by the following line: 172 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Steady-State HB Sources .HB TONES=1900MEG,1910MEG INTMODMAX=5 This specifies two fundamental frequencies: f [ tone = 1 ] = 1.9GHz and f [ tone = 2 ] = 1.91GHz . Their mixing product at 10 MHz can then be referenced using indices as f [ 2 ] – f [ 1 ] , while their 3rd order intermodulation product at 1.89 GHz can be referenced as 2f [ 1 ] – f [ 2 ] . Steady-state voltage and current sources are identified with the HB keyword according to <HB <mag <phase <harm <tone <modharm <modtone>>>>>>> The source is mathematically equivalent to a cosine signal source that follows the equation A cos ( ωt + φ) where A = mag ω = 2π harm ⋅ f [ tone ] + modharm ⋅ f [ mo dtone ] π φ = --------- ⋅ phase 180 Values for tone and modtone (an optional modulating tone) must be nonnegative integers that specify index values for the frequencies specified with the .HB TONES command. Values for harm (harmonic) and modharm (modulating tone harmonic) must be integers (negative values are OK) that specify harmonic indices. Example 1 The following example is a 1.0 Volt (peak) steady-state cosine voltage source, which is at the fundamental HB frequency with zero phase and with a zero volt DC value: Vsrc in gnd DC 0 HB 1.0 0 1 1 Example 2 The following example is a steady-state cosine power source with 1.0mW available power, which is implemented with a Norton equivalent circuit and a 50 ohm input impedance: HSPICE® RF User Guide Z-2007.03 173 Chapter 6: Testbench Elements Phase Differences Between HB and SIN Sources Isrc in gnd HB 1.0e-3 0 1 1 power=1 z0=50 Example 3 Five series voltage sources sum to produce a stimulus of five equally spaced frequencies at and above 2.44 GHz using modharm and modtone parameters. These are commensurate tones (an integer relation exists); therefore, you only need to specify two tones when invoking the HB analysis. .param Vin=1.0 .param f0=2440MEG .param deltaf=312.5K .param fcenter='f0 + 2.0*deltaf' Vrfa in ina HB 'Vin' 0 1 GHz Vrfb ina inb HB 'Vin' 0 1 2.4403125 GHz Vrfc inb inc HB 'Vin' 0 1 2.440 GHz Vrfd inc ind HB 'Vin' 0 1 2.4409375 GHz Vrfe ind gnd HB 'Vin' 0 1 GHz .HB tones=fcenter,deltaf intmodmax=5 1 $ 2.440625 1 -1 2 $ 1 -2 2 $ 1 +1 2 $ 1 +2 2 $ 2.44125 Phase Differences Between HB and SIN Sources The HB steady-state cosine source has a phase variation compared to the TRAN time-domain SIN source. The SIN source (with no offset, delay or damping) follows the equation: Equation 11 A sin ( ωt + φ) while the HB sources follow Equation 12 A cos ( ωt + φ) In order for the two sources to yield identical results it is necessary to align them by setting their phase values accordingly using: Equation 13 A cos ( ωt + φ) = A sin ( ωt + φ + 90° ) Equation 14 A sin ( ωt + φ) = A cos ( ωt + φ – 90° ) To specify sources with matching phase for HB and TRAN analysis, use a convention similar to: 174 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Behavioral Noise Sources ** Example #1 with equivalent HB and SIN sources ** SIN source is given +90 phase shift .param freq1=2400MEG Vin=1.0 Vsrc in gnd DC 0 HB 'Vin' 0 1 1 SIN(0 'Vin' 'freq1' 0 0 90) .HB tones=freq1 intmodmax=7 ** Example #2 with equivalent HB and SIN sources ** HB source is given -90 phase shift to align with SIN .param freq1=2400MEG Vin=1.0 Vsrc in gnd DC 0 HB 'Vin' -90 1 1 SIN(0 'Vin' 'freq1' 0) .HB tones=freq1 intmodmax=7 ** Example #3 with equivalent .HB and .TRAN sources ** SIN source is activated for HB using "TRANFORHB" .param freq1=2400MEG Vin=1.0 Vsrc in gnd DC 0 SIN(0 'Vin' 'freq1' 0) TRANFORHB=1 .HB tones=freq1 intmodmax=7 Behavioral Noise Sources In HSPICE RF, you can use the G element to specify noise sources. Frequency domain noise analyses (.NOISE, .HBNOISE, and .PHASENOISE) take these noise sources into account. You can attach noise sources to behavioral models. For example, you can use a G element with the VCCAP parameter to model a varactor, which includes a noise model. You can also simulate effects such as substrate noise, including its effect on oscillator phase noise. You can also use this G element syntax to simulate behavioral descriptions of substrate noise during any frequency domain noise analysis, which includes phase noise analysis. For example, gname node1 node2 noise=’noise_equation’ gname node1 node2 node3 node4 noise=’noise_equation’ The first line creates a simple two-terminal current noise source, whose value is described in A2/(Hz). The output noise generated from this noise source is: noise_equation*H Where H is the transfer function from the terminal pair (node1,node2) to the circuit output, where HSPICE RF measures the output noise. The second line produces a noise source correlation between the (node1,node2) and (node3,node4) terminal pairs. The resulting output noise is calculated as noise_equation*sqrt(H1*H2*); where, ■ H1 is the transfer function from (node1,node2) to the output ■ H2 is the transfer function from (node3,node4) to the output. HSPICE® RF User Guide Z-2007.03 175 Chapter 6: Testbench Elements Behavioral Noise Sources The noise_equation expression can involve node voltages and currents through voltage sources. For the PAC phasenoise simulation to evaluate the frequency-dependent noise, the frequency-dependent noise factor in the phasenoise must be expressed in between the parentheses. For example: gname node1 node2 noise = '(frequency_dependent_noise)* bias_dependent_noise' This is only true when the total noise can be expressed in this form and when the frequency-dependent noise can be evaluated in the PAC phasenoise simulation. You can also input the behavioral noise source as a noise table with the help of predefined Table() function. The Table() function takes two formats: ■ Noise table can be input directly through the Table() function. For example: gname node1 node2 noise = 'Table(arg1,f1,v1,f2,v2,......)' ■ The f1,v1,f2,v2,..... parameters describe the noise table. When arg1 == f1, the function returns v1. The arg1 can be an expression of either HERTZ, bias, or both. For example, arg1 = 'HERTZ * 1.0E+3'. ■ The noise table can be input through a .DATA structure: .DATA d1 + x y + f1 v1 + f2 v2 .ENDDATA gname node1 node2 noise = 'TABLE(arg1,d1)' The x, y parameters in the DATA structure are two placeholder strings that can be set to whatever you prefer even if they are in conflict with other parameters in the netlist. The arg1 parameter can be an expression of HERTZ and bias. When arg1 == f2, the function will return v2. Power Supply Current and Voltage Noise Sources You can implement the power supply noise source with G and E elements. The G element for the current noise source and the E element for the voltage noise source. As noise elements, they are two-terminal elements that represent a noise source connected between two specified nodes. 176 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Behavioral Noise Sources Syntax Expression form Gxxx node1 node2 noise=‘expression’ Exxx node1 node2 noise=‘expression’ The G noise element represents a noise current source and the E noise element represents a noise voltage source. The xxx parameter can be set with a value up to 1024 characters. The node1 and node2 are the positive and negative nodes that connect to the noise source. The noise expression can contain the bias, frequency, or other parameters. Data form Gxxx node1 node2 noise data=dataname Exxx node1 node2 noise data=dataname .data dataname + pname1 pname2 + freq1 noise1 + freq2 noise2 + ... .enddata The data form defines a basic frequency-noise table. The .DATA statement contains two parameters: frequency and noise to specify the noise value at each frequency point. The unit for frequency is hertz, and the unit for noise is A2/Hz (for G current noise source) or V2/Hz (for E voltage noise source). Example The following netlist shows a 1000 ohm resistor (g1) using a G element. The g1noise element, placed in parallel with the g1 resistor, delivers the thermal noise expected from a resistor. The r1 resistor is included for comparison: The noise due to r1 should be the same as the noise due to g1noise. * Resistor implemented using g-element v1 1 0 1 r1 1 2 1k g1 1 2 cur='v(1,2)*0.001' g1noise 1 2 + noise='4*1.3806266e-23*(TEMPER+273.15)*0.001' rout 2 0 1meg .ac lin 1 100 100 .noise v(2) v1 1 .end HSPICE® RF User Guide Z-2007.03 177 Chapter 6: Testbench Elements Function Approximations for Distributed Devices Function Approximations for Distributed Devices High-order rational function approximations constructed for distributed devices used at RF frequencies are obtained in the pole-residue form (also known as Foster canonical form). The popular method of recursive convolution also uses this form. HSPICE supports the pole-residue form for its frequency-dependent controlled sources (G and E elements). You can enter the pole-residue form directly without first converting to another form. Foster Pole-Residue Form for Transconductance or Gain The Foster pole-residue form for transconductance G(s) or gain E(s) has the form: ⎛ Ai A i∗ ⎞ -----------+ --------------⎜ ∑ ⎝ s – pi s – p ∗-⎟⎠ i N Equation 15 G ( s ) = k0 + k1 s + i=1 Where, ■ k0, k1 are real constants ■ residues Ai and poles pi are complex numbers (or real as a special case of complex ■ asterisk (*) denotes the expression's complex conjugate Advantages of Foster Form Modeling The advantages of Foster canonical form modeling are: 178 ■ models high-order systems. It can theoretically model systems having infinite poles without numerical problems. ■ equivalent to Laplace and Pole-zero models ■ popular method of recursive convolution uses this form. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Function Approximations for Distributed Devices G and E Element Syntax Transconductance G(s) form Gxxx n+ n+ (Re{A1}, + (Re{A2}, + (Re{A3}, + ... FOSTER in+ in- k0 Im{A1})/ (Re{p1}, Im{A2})/ (Re{p2}, Im{A3})/ (Re{p3}, k1 Im{p1}) Im{p2}) Im{p3}) FOSTER in+ in- k0 Im{A1})/ (Re{p1}, Im{A2})/ (Re{p2}, Im{A3})/ (Re{p3}, k1 Im{p1}) Im{p2}) Im{p3}) Gain E(s) form Exxx n+ n+ (Re{A1}, + (Re{A2}, + (Re{A3}, + ... In the above syntax, parenthesis , commas, and slashes are separators—they have the same meaning as a space. A pole-residue pair is represented by four numbers (real and imaginary part of the residue, then real and imaginary part of the pole). You must make sure that Re[pi]<0; otherwise, the simulations will certainly diverge. Also, it is a good idea to assure passivity of the model (for an N-port admittance matrix Y, Re{Y} should be positive-definite), or the simulation is likely to diverge). Example To represent a G(s) in the form, Equation 16 G ( s ) = 0.001 + 1 × 10 – 12 0.0008 ( 0.001 – j0.006 ) s + ---------------------------- + --------------------------------------------------------------------- + 10 8 10 s + 1 × 10 s – ( – 1 × 10 + j1.8 × 10 ) ( 0.001 + j0.006 ) -------------------------------------------------------------------8 10 s – ( – 1 × 10 – j1.8 × 10 ) You would input: G1 1 0 FOSTER 2 0 0.001 1e-12 +(0.0004, 0)/(-1e10, 0) (0.001, -0.006)/(-1e8, 1.8e10) HSPICE® RF User Guide Z-2007.03 179 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli Note: In the case of a real poles, half the residue value is entered, because it's essentially applied twice. In the above example, the first pole-residue pair is real, but we still write it as “A1/(s-p1)+A1/(s-p1)”; therefore, 0.0004 is entered rather than 0.0008. Complex Signal Sources and Stimuli To predict radio-frequency integrated circuit (RFIC) performance, some analyses require simulations that use representative RF signal sources. Among the representative sources available in HSPICE RF is the complex modulated RF source. Also known as the Vector Modulated source, it allows digital modulation of an RF carrier using in-phase and quadrature components created from a binary data stream. Vector-Modulated RF Source Digital RF waveforms are typically constructed by modulating an RF carrier with in-phase (I) and quadrature (Q) components. In HSPICE RF, this is accomplished using the Vector Modulated RF (VMRF) signal source. The VMRF signal source function is supported both for independent voltage and current sources (V and I elements), and with controlled sources (E, F, G, and H elements). ■ When used with independent sources, a baseband data stream can be input in binary or hexadecimal format, and the scheme used to divide the data into I and Q signals can be specified. ■ With controlled VMRF sources, the modulating I and Q signals can be separately specified with other signal sources (such as a PWL source) and then used as control inputs into the VMRF source. Implementation The VMRF source is a mathematical implementation of the following block diagram: 180 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli l(t) cos(wt) Data in Serial to Parallel S(t) sin(wt) Q(t) The following equation calculates the time and frequency domain stimuli from the quadrature modulated signal sources: Equation 17 s ( t ) = I ( t ) cos ( 2πf c t + φ0 ) – Q ( t ) sin ( 2πfct + φ0 ) The discrete ideal I (in-phase) and Q (quadrature) signal components are digital. Discrete values allow uniform scaling of the overall signal. HSPICE RF generates data streams for the I and Q signals based on interpreting the data string, breaking the data string into a binary representation, and then using the bit pairs to assign values for the I and Q data streams. For BPSK (binary phase shift keying) modulation, the discrete signals are scaled so that 2 2 I + Q = 1: Data In I Data Q Data 0 –1 ------2 –1 ------2 1 1 ------2 1 ------2 HSPICE® RF User Guide Z-2007.03 181 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli For QPSK (quadrature phase shift keying) modulation, the data stream is broken into bit pairs to form the correct I and Q values. This function is represented as the serial to parallel converter: Data In I Data Q Data 00 –1 ------2 –1 ------2 01 –1 ------2 1 ------2 10 1 ------2 –1 ------2 11 1 ------2 1 ------2 To generate a continuous-time waveform, the VMRF source takes the resulting digital I and Q data streams and passes them through ideal filters. Rectangular and Nyquist (raised-cosine) filter options are available. The output waveforms are therefore band-limited according to the specified data rate. Voltage and Current Source Elements The V and I elements can include VMRF signal sources that you can use to generate BPSK and QPSK waveforms. V and I Element Syntax Vxxx n+ n- VMRF <(> AMP=sa FREQ=fc PHASE=ph MOD=MOD + FILTER=FIL FILCOEF=filpar RATE=Rb BITSTREAM=data + <TRANFORHB=0/1> <)> Ixxx n+ n- VMRF <(> AMP=sa FREQ=fc PHASE=ph MOD=MOD + FILTER=FIL FILCOEF=filpar RATE=Rb BITSTREAM=data + <TRANFORHB=0/1> <)> 182 Parameter Description Vxxx Independent voltage source. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli Parameter Description Ixxx Independent current source. n+ n- Positive and negative controlled source connecting nodes. VMRF Keyword that identifies and activates the Vector Modulated RF signal source. AMP Signal amplitude (in volts or amps). FREQ Carrier frequency in hertz. Set fc=0.0 to generate baseband I/Q signals. For harmonic balance analysis, the frequency spacing must coincide with the .HB TONES settings. PHASE Carrier phase (in degrees). If fc=0.0, ■ ■ ■ MOD One of the following keywords identifies the modulation method used to convert a digital stream of information to I(t) and Q(t) variations: ■ ■ FILTER ph=0 and baseband I(t) is generated ph=-90 and baseband q(t) is generated Otherwise, s ( t ) = I ( t ) cos ( φ0 ) – Q ( t ) sin ( φ0 ) BPSK (binary phase shift keying) QPSK (quadrature phase shift keying) One of the following keywords identifies the method used to filter the I and Q signals before modulating the RF carrier signal: ■ ■ COS (raised cosine Nyquist filter) RECT (rectangular filtering) FILCOEF Filter parameter for the COS filter: 0 ≤filpar ≤1 RATE Bit rate for modulation (bits per second). ■ For BPSK modulation, the data rate and the symbol rate are the same. ■ For QPSK modulation, the symbol rate is half the data rate. The Rb value must be greater than zero. HSPICE® RF User Guide Z-2007.03 183 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli Parameter Description BITSTREAM A binary (b) or hexadecimal (h) string that represents an input data stream. Valid data string characters are: ■ 0 or 1 for binary (b) mode. 0, 1, 2, 3, 4, 5, 6, 7, 8, 9, A, B, C, D, E, F, a, b, c, d, e, or f for hexadecimal (h) mode. For example: ■ ■ ■ 01010011b (binary) 0F647A30E9h (hexadecimal) You can also use the standard V source and I source options for non-transient simulations (such as DC=val and AC=mag,ph) a with the VMRF source. Example BITSTREAM=01010010011100b data 1/dr BPSK I and Q Signals .707 1/dr 184 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli QPSK I Signal .707 1/dr QPSK Q Signal .707 1/dr The Rb parameter represents the data rate. The associated symbol rate represents how fast the I and Q data streams change. The period for each bit of data is: Equation 18 1T b = ----Rb The symbol rate depends on whether you select BPSK or QPSK modulation: ■ For BPSK, the symbol rate is the same as the data rate: S ■ R BPSK = Rb For QPSK modulation, two bits are used to create each symbol so the symbol rate is half the data rate. R S QPSK R = -----b2 The period for each symbol is computed as: Equation 19 1T s = ---Rs This value is necessary for establishing the characteristics of Nyquist filters. HSPICE® RF User Guide Z-2007.03 185 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli The following equation calculates the raised cosine (COS) filter response: 1–α f ≤-----------2T s Equation 20 H rc ( f ) = ∫ Ts 0 2 πT s 1–α T s cos -------- ⎛ f – ------------⎞ 2α ⎝ 2T s ⎠ 1–α 1+α ------------ ≤ f ≤-----------2T s 2T s 1+a f > -----------2T s The VMRF signal source is designed primarily for TRAN and HB analyses, and can generate baseband signals. You can also specify DC and AC values as with any other HSPICE signal source: ■ In DC analysis, the VMRF source is a constant DC source. ■ In AC analysis, the source is a short or an open, unless you specify an AC value. ■ In HB analysis, you must specify .OPTION TRANFORHB on the source statement line. The TRANFORHB option supports the VMRF signal source as well as the SIN, PULSE, and PWL sources. The VMRF quadrature signal source typically involves an HF carrier signal that is modulated with a baseband signal on a much different time scale. You must set source and simulation control parameters appropriately to avoid timeconsuming simulations in both the time and frequency domains. E, F, G, and H Element Statements For E, F, G, and H elements, you can use the VMRF function to modulate I(t) and Q(t) signals with a RF carrier signal. The I and Q signal are driven by PWL sources that might be generated by an external tool, such as MATLAB. The PWL source accepts a text file containing time and voltage (or current) pairs. When the VMRF function is used with controlled sources, it is anticipated that the in-phase (I) and quadrature (Q) signals are not digital, but continuous-time analog signals. The VMRF function therefore includes no filtering, and merely serves to create the complex modulation on the RF carrier. Exxx n+ n- <VCVS> VMRF <(> Iin+ Iin- Qin+ Qin- FREQ=fc + PHASE=ph <SCALE=A> <)> Fxxx n+ n- <CCCS> VMRF <(> VI VQ FREQ=fc PHASE=ph + <SCALE=A> <)> 186 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli Gxxx n+ n- <VCCS> VMRF <(> Iin+ Iin- Qin+ Qin- FREQ=fc + PHASE=ph <SCALE=A> <)> Hxxx n+ n- <CCVS> VMRF <(> VI VQ FREQ=fc PHASE=ph + <SCALE=A> <)> Parameter Description Exxx Voltage-controlled voltage source. Fxxx Current-controlled current source. Gxxx Voltage-controlled current source. Hxxx Current-controlled current source. VCVS Keyword for voltage-controlled voltage source. CCCS Keyword for current-controlled current source. VCCS Keyword for voltage-controlled current source. CCVS Keyword for current-controlled current source. n+ n- Positive and negative controlled source connecting nodes. VMRF Keyword that identifies and activates the vector-modulated RF signal source. Iin+ Iin- Node names for input I(t) signal. Qin+ Qin- Node names for input Q(t) signal. VI VQ FREQ Carrier frequency in Hertz. Set fc=0.0 to generate baseband I/Q signals. PHASE Carrier phase (in degrees). If fc=0.0, ■ ■ SCALE ΗΣΠΙΧΕ→ΡΦΥσερΓυιδε Z-2007.03 ph=0 and baseband I(t) is generated ph=-90 and baseband Q(t) is generated Unit-less amplitude scaling parameter. 187 Chapter 6: Testbench Elements Complex Signal Sources and Stimuli Example Emod1 inp1 inn1 VMRF It_plus It_neg Qt_plus Qt_neg + freq=1g phase=0 scale=1.5 File-Driven PWL Source Vxxx n1 n2 PWL PWLFILE='filename' <col1, <col2>> <R=repeat> + <TD=delay> <options> Ixxx n1 n2 PWL PWLFILE='filename' <col1, <col2>> <R=repeat> + <TD=delay> <options> 188 Parameter Description Vxxx Independent voltage source. Ixxx Independent current source. n1 n2 Positive and negative terminal node names. PWL Keyword for piecewise linear. PWLFILE Text file containing the PWL data consisting of time and voltage (or current) pairs. This file should not contain a header row, unless it is a comment. The PWL source data is obtained by extracting col1 and col2 from the file. col1, <col2> Time values are in col1 and voltage (or current) values are in col2. By default, col1=1 and col2=2. R Repeat function. When an argument is not specified, the source repeats from the beginning of the function. The argument repeated is the time, in seconds, which specifies the start point of the waveform being repeat. The repeat time must be less than the greatest time point in the file. TD Time delay, in seconds, of the PWL function. options Any standard V or I source options. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements SWEEPBLOCK in Sweep Analyses Example Vit It_plus It_neg PWL PWLFILE=’Imod.dat’ SWEEPBLOCK in Sweep Analyses You can use the .SWEEPBLOCK statement to specify complicated sweeps. Sweeps affect: ■ DC sweep analysis ■ Parameter sweeps around TRAN, AC, or HB analyses ■ Frequency values used in AC or HBAC analyses Currently, HSPICE supports the following types of sweeps: ■ ■ ■ Linear sweeps: sweeps a variable over an interval with a constant increment. The syntax is one of the following: • variable start stop increment • variable lin npoints start stop Logarithmic sweeps: sweeps a variable over an interval. To obtain each point, this sweep multiplies the previous point by a constant factor. You can specify the factor as a number of points per decade or octave as in: • variable dec npoints start stop • variable oct npoints start stop Point sweeps: a variable takes on specific values that you specify as a list. The syntax is: variable poi npoints p1 p2 … ■ Data sweeps: a .DATA statement identifies the swept variables and their values. The syntax is: data=dataname You can use the SWEEPBLOCK feature to combine linear, logarithmic, and point sweeps, which creates more complicated sets of values over which a variable is swept. The .TRAN, .AC, .DC, and .HB commands can specify SWEEPBLOCK=blockname as a sweep instead of LIN, DEC, OCT, and so forth. Also, you can use SWEEPBLOCK for frequency sweeps with the .AC, .HBAC, .PHASENOISE, and .HBNOISE commands. HSPICE® RF User Guide Z-2007.03 189 Chapter 6: Testbench Elements SWEEPBLOCK in Sweep Analyses All commands that can use SWEEPBLOCK must refer to the SWEEPBLOCK sweep type. In addition, you must specify SWEEPBLOCK as one of the syntax types allowed for frequency sweeps with the .HBAC, .PHASENOISE, and .HBNOISE commands. Input Syntax The SWEEPBLOCK feature creates a sweep whose set of values is the union of a set of linear, logarithmic, and point sweeps. To specify the set of values in the SWEEPBLOCK, use the .SWEEPBLOCK command. This command also assigns a name to the SWEEPBLOCK. For example, .SWEEPBLOCK swblockname sweepspec [sweepspec + [sweepspec […]]]] You can use SWEEPBLOCK to specify DC sweeps, parameter sweeps, AC and HBAC frequency sweeps, or wherever HSPICE accepts sweeps. You can specify an unlimited number of sweepspec parameters. Each sweepspec can specify a linear, logarithmic, or point sweep by using one of the following forms: start stop increment lin npoints start stop dec npoints start stop oct npoints start stop poi npoints p1 p2 … Example The following example specifies a logarithmic sweep from 1 to 1e9 with more resolution from 1e6 to 1e7: .sweepblock freqsweep dec 10 1 1g dec 1000 1meg 10meg Using SWEEPBLOCK in a DC Parameter Sweep To use the sweepblock in a DC parameter sweep, use the following syntax: .DC sweepspec [sweepspec [sweepspec]] Each sweepspec can be a linear, logarithmic, point, or data sweep, or it can be in the form: variable SWEEPBLOCK=swblockname 190 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Clock Source with Random Jitter The SWEEPBLOCK syntax sweeps the specified variable over the values contained in the SWEEPBLOCK. Example .dc vin1 0 5 0.1 vin2 sweepblock=vin2vals Using in Parameter Sweeps in TRAN, AC, and HB Analyses To use the sweepblock in parameter sweeps on .TRAN, .AC, and .HB commands, and any other commands that allow parameter sweeps, use the following syntax: variable sweepblock=swblockname Example 1 .tran 1n 100n sweep rout sweepblock=rvals AC and HBAC analysis frequency sweeps can use sweepblock=swblockname to specify the frequency values. Example 2 .ac sweepblock=freqsweep Limitations ■ You cannot use recursive SWEEPBLOCK specifications. That is, a .SWEEPBLOCK command cannot refer to another SWEEPBLOCK to build its list of values. ■ You cannot include data sweeps in a .SWEEPBLOCK statement. Clock Source with Random Jitter In many applications involving signal integrity, RF, analog, and mixed-signal design, it is desirable to have an ideal signal source, such as a sine wave or square wave, that also includes a non-ideal random drift in phase (jitter). Such a source is useful for representing non-ideal clock sources during time-domain transient simulation. Modeling jitter in this way can be used to examine eyediagram behavior or study how jitter may propagate through a circuit or system. A source with jitter is useful for representing non-ideal clock sources during time-domain transient simulation. HSPICE® RF User Guide Z-2007.03 191 Chapter 6: Testbench Elements Clock Source with Random Jitter The PERJITTER option allows you to add periodic jitter to SIN, COS and PULSE time domain sources. Syntax of SIN, COS, and Pulse Sources The syntax of SIN source is: Vxxx n+ n- SIN <(> vo va <freq <td <q <j >>>> <)> + <PERJITTER=val SEED=val>> Ixxx n+ n- SIN <(> vo va <freq <td <q <j >>>> <)> + <PERJITTER=val SEED=val>> Parameter Description Vxxx Independent voltage source. Ixxx Independent current source. PERJITTER Period jitter PWL Keyword for piecewise linear. PWLFILE Text file containing the PWL data consisting of time and voltage (or current) pairs. This file should not contain a header row, unless it is a comment. The PWL source data is obtained by extracting col1 and col2 from the file. col1, <col2> Time values are in col1 and voltage (or current) values are in col2. By default, col1=1 and col2=2. R Repeat function. When an argument is not specified, the source repeats from the beginning of the function. The argument repeated is the time, in seconds, which specifies the start point of the waveform being repeat. The repeat time must be less than the greatest time point in the file. TD Time delay, in seconds, of the PWL function. options Any standard V or I source options. The sine wave behavior following the td time delay now becomes Equation 21 192 V(t) + e – ( t – td ) ⋅ θ = V0 + Va ⋅ π sin 2πf 0 ( t – t d ) + --------- ϕ + φt – d d 180 HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements Clock Source with Random Jitter The Syntax of COS source is: Vxxx n+ n- COS <(> vo va <freq <td <q <j >>>> <)> <PERJITTER=val <SEED=val>> Ixxx n+ n- COS <(> vo va <freq <td <q <j >>>> <)> <PERJITTER=val <SEED=val>> The new cosine wave becomes Equation 22 V(t) + e – ( t – td ) ⋅ θ = V0 + Va ⋅ π cos 2 πf 0 ( t – t d + x ( t ) ) + --------- ϕ 180 The syntax for the PULSE source is: Vxxx n+ n- PU<LSE> <(>v1 v2 <td <tr <tf <pw <per>>>>> <)> + <PERJITTER=val SEED=val>> Ixxx n+ n- PU<LSE> <(>v1 v2 <td <tr <tf <pw <per>>>>> <)> + <PERJITTER=val SEED=val>> The effect of jitter on the PULSE source results in random shifts of the rise and fall transitions that takes place at RISE edge: td + n ⋅ T 0 ≤t ≤td + tr + n ⋅ T 0 FALL edge: td + pw + n ⋅ T 0 ≤t ≤td + pw + tf + n ⋅ T 0 The jitter effect is equivalent to introducing random shifts in the period T 0 consistent with the 1st order jitter model based on Period Jitter. A Gaussian random number generator computes the time deviation x ( t ) after each leading edge of the clock sources. For flexibility, the SEED parameter (integer) is supported for generating different random number sequences when different SEED integers are used for initialization. SEED does not set a fixed time deviation. It only changes the sequence of random samples. By HSPICE (Monte Carlo) convention, the default value for SEED is -1. An interpretation of PERJITTER is to view it as causing each period of the PULSE/SIN/COS to be a random variable T j , where period T j will have a Gaussian distribution about the (mean) given period value of T 0 . The standard deviation of this Gaussian is the PERJITTER value (it is considered RMS period jitter), which results in a bell curve distribution centered about period T 0 . HSPICE® RF User Guide Z-2007.03 193 Chapter 6: Testbench Elements Clock Source with Random Jitter Apply the following considerations when using PERJITTER: ■ T j should be forced to be between: 0 < T j < 2 ⋅ T 0, since period cannot go negative, and the curve should be symmetrical. ■ It is reasonable to require that2 ⋅ PERJITTER < T 0. Otherwise, the jitter would result in very large period changes, and many would be T j < 0 . ■ 194 To establish a waveform reference, the first period should be T 0 (i.e., no jitter in the first period). This helps to establish good eye diagrams. HSPICE® RF User Guide Z-2007.03 Chapter 6: Testbench Elements References References [1] L.J. Greenstein and M.Shafi, Microwave Digital Radio, IEEE Press, 1988. [2] N. Sheikholeslami and P. Kabal, “A Family of Nyquist Filters Based on Generalized Raised-Cosine Spectra,” Proceedings of the 19th Biennial Symposium on Communications (Kingston, Ontario), pages 131-135, June 1998. [3] IEEE Standard Definitions of Physical Quantities for Fundamental Frequency and Time Metrology - Random Instabilities, IEEE Std. 11391999. [4] A. van der Ziel, Noise in Solid State Devices and Circuits, John Wiley & Sons, © 1986. [5] A. Demir, A. Mehrotra, and J. Roychowdhury, "Phase noise in oscillators: A unifying theory and numerical methods for characterization," IEEE Trans. Circuits Syst. I, vol. 47, pp. 655-674, May 2000. [6] A. Hajimiri, S. Limotyrakis, and T.H. Lee, "Jitter and phase noise in ring oscillators," IEEE J. Solid-State Circuits, vol. 34, no. 6, pp. 790-804, June 1999. [7] Jitter Analysis Techniques for High Data Rates, Application Note 1432, Agilent Technologies, Feb. 2003.[6] Characterization of Clocks and Oscillators, NIST Technical Note 1337, National Institute of Standards and Technology. HSPICE® RF User Guide Z-2007.03 195 Chapter 6: Testbench Elements References 196 HSPICE® RF User Guide Z-2007.03 7 7 Steady-State Harmonic Balance Analysis Describes how to use harmonic balance analysis for frequency-driven, steadystate analysis. HSPICE RF provides several analyses that support the simulation and analysis of radio-frequency integrated circuits (RFICs). These analyses provide simulation capabilities that are either much more difficult to perform, or are not practically possible by using standard HSPICE analyses. The RF analyses include: ■ Harmonic Balance (HB) for frequency-domain, steady-state analysis, see Harmonic Balance Analysis on page 198. ■ Shooting Newton (SN) for frequency or time domain steady state analysis, see Chapter 8, Steady-State Shooting Newton Analysis plus spectrum analysis specific to the SN analysis (see Shooting Newton with Fourier Transform (.SNFT). ■ Harmonic Balance oscillator analysis (HBOSC), see Harmonic Balance Analysis for Frequency of Oscillation on page 229. ■ Shooting Newton oscillator analysis (SNOSC), see Oscillator Analysis Using Shooting Newton (.SNOSC) on page 236. ■ Harmonic Balance AC (HBAC) for periodic AC analysis, see Chapter 10, Large Signal Periodic AC, Transfer Function, and Noise Analyses, Multitone Harmonic Balance AC Analysis (.HBAC) on page 257. ■ Shooting Newton AC analysis, see Shooting Newton AC Analysis (.SNAC) on page 263. ■ Harmonic Balance Noise (HBNOISE) for periodic, time-varying AC noise analysis (see Chapter 10, Large Signal Periodic AC, Transfer Function, and Noise Analyses). HSPICE® RF User Guide Z-2007.03 197 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis ■ Shooting Newton noise analysis, see Shooting Newton Noise Analysis (.SNNOISE) on page 275. ■ Harmonic balance transfer functions, see Multitone Harmonic Balance Transfer Function Analysis (.HBXF) on page 287. ■ Shooting Newton transfer functions, see Shooting Newton Transfer Function Analysis (.SNXF) on page 291 ■ Frequency translation S-parameter extraction for describing N-port circuits that exhibit frequency translation effects (see Frequency Translation SParameter (HBLIN) Extraction on page 298). ■ Envelope Analysis (ENV) (see Chapter 12, Envelope Analysis). You can use steady-state analysis on a circuit if it contains only DC and periodic sources. These analyses assume that all “start-up” transients have completely died out with only the steady-state response remaining. Sources that are not periodic or DC are treated as zero-valued in these analyses. Harmonic Balance Analysis Harmonic balance analysis (HB) is a frequency-domain, steady-state analysis technique. In HSPICE RF, you can use this analysis technique on a circuit that is excited by DC and periodic sources of one or more fundamental tones. The solution that HB finds is a set of phasors for each harmonic signal in the circuit. You can think of this solution as a set of truncated Fourier series. HSPICE RF allows you to specify the solution spectrum to use in an analysis. HB analysis then finds the set of phasors at these frequencies that describes the circuit response. The result is a set of complex valued Fourier series coefficients that represent the waveforms at each node in the circuit. Linear circuit elements are evaluated in the frequency domain, while nonlinear elements are evaluated in the time domain. The nonlinear response is then transformed to the frequency domain where it is added to (or “balanced” with) the linear response. The resulting composite response satisfies KCL and KVL (Kirchoff's current and voltage laws) when the circuit solution is found. Typical applications include performing intermodulation analysis, oscillator analysis, and gain compression analysis, on amplifiers and mixers. HB analysis also serves as a starting point for periodic AC and noise analyses. 198 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Harmonic Balance Equations We can write Kirchoff's current law in the time domain as: t Equation 23 f ( v, t ) = i ( v ( t ) ) + d q ( v ( t ) ) + ∫ y ( t – τ )v ( τ ) dτ + i s ( t ) = 0 dt –∞ ■ i(v(t)) represents the resistive currents from nonlinear devices ■ q represents the charges from nonlinear devices ■ y represents the admittance of the linear devices in the circuit ■ is represents the vector of independent current sources ■ v is a variable that represents the circuit unknowns, both node voltages and branch currents, and f(v,t) is an error term that goes to zero when Kirchoff's current law is satisfied. Transforming this equation to the frequency domain results in: Equation 24 F ( V ) = I ( V ) + ΩQ ( V ) + Y ( ω)V + I s = 0 Note: Time-differentiation is transformed to multiplication by jω terms (which make up the Ω matrix) in the frequency domain. The convolution integral is transformed to a simple multiplication. The Y matrix is the circuit’s modified nodal admittance matrix. All terms above are vectors, representing the circuit response at each analysis frequency. The following equation shows the vector of (complex-valued) unknowns in the frequency domain for a circuit with K analysis frequencies and N unknowns. Equation 25 V = V ( 1, 0) V ( 1, 1) …V ( 1, K – 1) V ( 2, 0) …V ( N, K – 1) HSPICE RF finds the unknown vector (V), which satisfies the system of nonlinear equations shown in the equation above. This is done via the NewtonRaphson technique by using either a direct solver to factor the Jacobian matrix, or an indirect solver. The indirect solver available in HSPICE RF is the Generalized Minimum Residual (GMRES) Solver, a Krylov technique, and uses a matrix-implicit algorithm. HSPICE® RF User Guide Z-2007.03 199 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Features Supported HB supports the following features: ■ All existing HSPICE RF models. ■ Unlimited number of independent input tones. ■ Sources with multiple HB specifications. ■ SIN, PULSE, VMRF, and PWL sources with TRANFORHB=1. Prerequisites and Limitations The following prerequisites and limitations apply to HB: ■ Requires one .HB statement. ■ Treats sources without a DC, HB, or TRANFORHB description as a zerovalue for HB unless the sources have a transient description, in which case, the time=0 value is used as a DC value. Input Syntax Without SS_TONE .HB TONES=<F1> [<F2> <...> <FN>] [SUBHARMS=SH] + <NHARMS=<H1>, <H2> <...> <HN>> <INTMODMAX=n> + [SWEEP parameter_sweep] With SS_TONE .HB TONES=<F1> [<F2> <...> <FN>] + <NHARMS=<H1>, <H2> <...> <HN>> <INTMODMAX=n> + <SS_TONE=n> [SWEEP parameter_sweep] 200 Parameter Description TONES Fundamental frequencies. SUBHARMS Allows subharmonics in the analysis spectrum. The minimum nonDC frequency in the analysis spectrum is f/subharms, where f is the frequency of oscillation. HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Parameter Description NHARMS Number of harmonics to use for each tone. Must have the same number of entries as TONES. You must specify NHARMS, INTMODMAX, or both. INTMODMAX INTMODMAX is the maximum intermodulation product order that you can specify in the analysis spectrum. You must specify NHARMS, INTMODMAX, or both. SS_TONE Small-signal tone number for HBLIN analysis. The value must be an integer number. The default value is 0, indicating that no small signal tone is specified. For additional information, see Frequency Translation S-Parameter (HBLIN) Extraction on page 298. SWEEP Type of sweep. You can sweep up to three variables. You can specify either LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, OPTIMIZE, or MONTE. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ ■ ■ ■ LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn DATA=dataname OPTIMIZE=OPTxxx MONTE=val HB Analysis Spectrum The NHARMS and INTMODMAX input parameters define the spectrum. ■ If INTMODMAX=N, the spectrum consists of all f=a*f1 + b*f2 + ... + n*fn frequencies so that f>=0 and |a|+|b|+...+|n|<=N. The a,b,...,n coefficients are integers with absolute value <=N. ■ If you do not specify INTMODMAX, it defaults to the largest value in the NHARMS list. ■ If entries in the NHARMS list are > INTMODMAX, HSPICE RF adds the m*fk frequencies to the spectrum, where fk is the corresponding tone, and m is a value <= the NHARMS entry. HSPICE® RF User Guide Z-2007.03 201 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Example 1 .hb tones=f1, f2 intmodmax=1 The resulting HB analysis spectrum={dc, f1, f2} Example 2 .hb tones=f1, f2 intmodmax=2 The resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2} Example 3 .hb tones=f1, f2 intmodmax=3 The resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2, 2*f1+f2, 2*f1-f2, 2*f2+f1, 2*f2-f1, 3*f1, 3*f2} Example 4 .hb tones=f1, f2 nharms=2,2 The resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2} Example 5 hb tones=f1, f2 nharms=2,2 intmodmax=3 The resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2, 2*f1-f2, 2*f1+f2, 2*f2-f1, 2*f2+f1} Example 6 .hb tones=f1, f2 nharms=5,5 intmodmax=3 The resulting HB analysis spectrum={dc, f1, f2, f1+f2, f1-f2, 2*f1, 2*f2, 2*f1-f2, 2*f1+f2, 2*f2-f1, 2*f2+f1, 3*f1, 3*f2, 4*f1, 4*f2, 5*f1, 5*f2} 202 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis HB Analysis Options The following table lists the .OPTION command options specific to HB analysis. Table 16 HB Analysis Options Option Description HBCONTINUE Specifies whether to use the sweep solution from the previous simulation as the initial guess for the present simulation. ■ ■ HBJREUSE HBCONTINUE=1 (default): Use solution from previous simulation as the initial guess. HBCONTINUE=0: Start each simulation in a sweep from the DC solution. Controls when to recalculate the Jacobian matrix: ■ HBJREUSE=0 recalculates the Jacobian matrix at each iteration. ■ HBJREUSE=1 reuses the Jacobian matrix for several iterations, if the error is sufficiently reduced. The default is 0 if HBSOLVER=1 or 2, or 1 if HBSOLVER=0. HBJREUSETOL Determines when to recalculate Jacobian matrix (if HBJREUSE=1). The percentage by which HSPICE RF must reduce the error from the last iteration so you can use the Jacobian matrix for the next iteration. Must be a real number, between 0 and 1. The default is 0.05. HBKRYLOVDIM Dimension of the Krylov subspace that the Krylov solver uses. Must be an integer, greater than zero. Default is 40. HBKRYLOVTOL The error tolerance for the Krylov solver. Must be a real number, greater than zero. The default is 0.01. HBLINESEARCHFAC The line search factor. If Newton iteration produces a new vector of HB unknowns with a higher error than the last iteration, then scale the update step by HBLINESEARCHFAC, and try again. Must be a real number, between 0 and 1. The default is 0.35. HSPICE® RF User Guide Z-2007.03 203 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Table 16 HB Analysis Options (Continued) Option Description HBMAXITER Specifies the maximum number of Newton-Raphson iterations that the HB engine performs. Analysis stops when the number of iterations reaches this value. The default is 10000. HBSOLVER Specifies a preconditioner to solve nonlinear circuits. ■ ■ ■ 204 HBSOLVER=0: invokes the direct solver. HBSOLVER=1 (default): invokes the matrix-free Krylov solver. HBSOLVER=2: invokes the two-level hybrid timefrequency domain solver. HBTOL The absolute error tolerance for determining convergence. Must be a real number that is greater than zero. The default is 1.e-9. LOADHB LOADHB=’filename’ loads the state variable information contained in the specified file. These values are used to initialize the HB simulation. SAVEHB SAVEHB=’filename’ saves the final state (that is, the no sweep point or the steady state of the first sweep point) variable values from a HB simulation in the specified file. This file can be loaded as the starting point for another simulation by using a LOADHB option. TRANFORHB ■ TRANFORHB=1: forces HB to recognize V/I sources that include SIN, PULSE, VMRF, and PWL transient descriptions, and to use them in analysis. However, if the source also has an HB description, analysis uses the HB description instead. ■ TRANFORHB=0: forces HB to ignore transient descriptions of V/I sources, and to use only HB descriptions. To override this option, specify TRANFORHB in the source description. HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Harmonic Balance Output Measurements This section explains the harmonic balance output measurements you receive after HSPICE runs an HB simulation. Harmonic Balance Signal Representation The HB cosine sources can be interpreted in real/imaginary and polar formats according to: v ( t ) = A cos ( αt + φ) = Re {Ae j ( αt + φ) jφ jωt }= Re {Ae e } jφ Equation 26 = Re {Ae [ cos ( αt ) + j sin ( αt ) ] } = Re {[ V R + jV I ] [ cos ( αt ) + j sin ( αt ) ] } = V R cos ( αt ) – V I sin ( at ) = A cos ( φ) cos ( αt ) – A sin ( φ) sin ( αt ) Note that real/imaginary and polar formats are related with the standard convention: Equation 27 V R + jV I = Ae jφ V R = A cos ( φ) V I = A sin ( φ) A = 2 2 VR + VI V tan φ = -----IVR The result of HB analysis is a complex voltage (current) spectrum at each circuit node (or specified branch). Let a[i] be the real part and b[i] be the imaginary part of the complex voltage at the ith frequency index. Conversion to a steady-state time-domain waveform is given by the Fourier series expansion: HSPICE® RF User Guide Z-2007.03 205 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Equation 28 v(t) = a[0] + a[1]*cos(2πf[1]*t) – b[1]*sin(2πf[1]*t) + a[2]*cos(2πf[2]*t) – b[2]*sin(2πf[2]*t) + a[3]*cos(2πf[3]*t) – b[3]*sin(2πf[3]*t) +... + a[N]*cos(2πf[N]*t) – b[N]*sin(2πf[N]*t) Where: ■ v(t) is the resulting time domain waveform. ■ N+1 is the total number of harmonics (including DC) in the frequency domain spectrum of the *.hb0 file (the zero-th data point represents DC). ■ a[i] is the real component at the ith frequency ■ b[i] is the imaginary component at the ith frequency ■ f[i] is the ith frequency value (with i=0 representing the zero frequency DC term). These frequencies need not be harmonically related. This frequency domain (Fourier coefficient) representation can be converted into a steady-state time domain waveform output representation by using the .PRINT or .PROBE HBTRAN output option or by invoking the To Time Domain function on complex spectra within CosmosScope. Output Syntax This section describes the syntax for the HB .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT HB TYPE(NODES or ELEM)[INDICES] 206 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis .PROBE HB TYPE(NODES or ELEM)[INDICES] Parameter Description TYPE(NODES or ELEM) Specifies a harmonic type node or element. TYPE can be one of the following: ■ ■ ■ ■ Voltage type – V = voltage magnitude and phase in degrees VR = real component VI = imaginary component VM = magnitude VP - Phase in degrees VPD - Phase in degrees VPR - Phase in radians VDB - dB units VDBM - dB relative to 1 mV Current type – I = current magnitude and phase in degrees IR = real component II = imaginary component IM = magnitude IP - Phase in degrees IPD - Phase in degrees IPR - Phase in radians IDB - dB units IDBM - dB relative to 1 mV Power type – P Frequency type – ‘HERTZ[i]’ (for single tone analysis), ‘HERTZ[i][j]’ (for two-tone analysis) , ‘HERTZ[i][j][k]’ (for 3-tone analysis), etc. You must specify the harmonic index integer for the HERTZ keyword. The frequency of the specified harmonics is dumped. NODES or ELEM can be one of the following: ■ ■ ■ HSPICE® RF User Guide Z-2007.03 Voltage type – a single node name (n1), or a pair of node names, (n1,n2) Current type – an element name (elemname) Power type – a resistor (resistorname) or port (portname) element name. 207 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Parameter Description INDICES Index to tones in the form [n1, n2, ..., nN], where nj is the index of the HB tone and the HB statement contains N tones. If INDICES is used, then wildcards are not supported. HB data can be transformed into the time domain and output using the following syntax: .PRINT hbtran ov1 <ov2 ... > .PROBE hbtran ov1 <ov2 ... > Where ov1 ... are the output variables to print or probe. Calculating Power Measurements After HB Analyses Two types of power measurements are available: dissipated power in resistors and delivered power to port elements. The following subtle differences between these two measurements are described in this section. Power Dissipated in a Resistor All power calculations make use of the fundamental phasor power relationship given as the following equation, where voltage V and current I are complex phasors given in peak values (not rms, nor peak-to-peak): Equation 29 1 P rms = --- Re {VI∗ } 2 In the case of a simple resistor, its current and voltage are related according to Vn=InR. The power dissipated in a resistor of (real) value R at frequency index n is then given by: 2 Equation 30 Vn P rms ( resistor ) [ n ] = ---------2R Power Delivered to a Port Element The port element can be either a source or sink for power. You can use a special calculation that computes the power flowing into a port element even if the port element itself is the source of that power. In the following figure is a 208 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis port element connected to a circuit (the port element may or may not include a voltage source). Figure 21 Port Element Zo In + + Vs Port Element Remainder Of Circuit Vn - Let Vn be the (peak) voltage across the terminals of the port element (at frequency index n). Let In be the (peak) current into the (1st) terminal of the port element (at frequency index n). Let Zo be the impedance value of the z0 port element. Then, the power wave flowing into the terminals of the port element (at frequency index n) can be computed according to: Equation 31 1 Vn + Zo In P in [ n ] = --- ---------------------2 2 Z o 2 This power expression remains valid whether or not the port element includes an internal voltage source at the same frequency. If the port element includes a voltage source at the same frequency, you can use this power calculation to compute the magnitude of the related large-signal scattering parameters. If you expand the preceding formula, the power delivered to a port element with (real) impedance Zo is given by 2 Equation 32 2 2 1 ⎧ Vn + Zo In 1 P rms ( port ) [ n ] = --- ⎨ ----------------------------------- + --- Re {V n I∗n 2⎩ 2 4Z o ⎫ }⎬ ⎭ This power value represents the power incident upon and delivered to the port element's load impedance (Zo) due to other power sources in the circuit, and due to reflections of its own generated power. HSPICE® RF User Guide Z-2007.03 209 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis If the port element is used as a load resistor (no internal source), the preceding equation reduces to that for the simple resistor. If you used the port element as a power source (with non-zero available power, i.e. a non-zero Vs) and it is terminated in a matched load (Zo), the port power measurement returns 0 W, because no power is reflected. You can request power measurements in the form of complete spectra or in the form of scalar quantities that represent power at a particular element. To request a complete power spectrum, use the following syntax. .PRINT HB P(Elem) .PROBE HB P(Elem) To request a power value at a particular frequency tone, use the following syntax: .PRINT HB P(Elem)[<n1<,n2<n3,...>>>] .PROBE HB P(Elem)[<n1<,n2<,n3,...>>>] The Elem is the name of either a Resistor (R) or Port (P) element, and n1,n2, and n3 are integer indices used for selecting a particular frequency in the Harmonic Balance output spectrum. Example 1 Prints a table of the RMS power (spectrum) dissipated by resistor R1. .PRINT HB P(R1) Example 2 Outputs the RMS power dissipated by resistor R1 at the fundamental HB analysis frequency following a one-tone analysis. .PROBE HB P(R1)[1] Example 3 Prints the power dissipated by resistor R1 at DC following a one-tone analysis. .PRINT HB P(R1)[0] Example 4 Outputs the RMS power dissipated by resistor R1 at the (low-side) 3rd order intermodulation product following an HB two-tone analysis. 210 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis .PROBE HB P(R1)[2,-1] Example 5 Prints the RMS power dissipated by resistor R1 at the (high-side) 3rd order intermodulation product following an HB two-tone analysis. .PRINT HB P(R1)[-1,2] Example 6 Outputs the RMS power (spectrum) delivered to port element Pload. .PROBE HB P(Pload) Example 7 Prints the RMS power delivered to port element Pload at the fundamental HB analysis frequency following a one-tone analysis. .PRINT HB P(Pload)[1] $ Example 8 Outputs the RMS power delivered to port element Pload at the (low-side) 3rd order intermodulation product following an HB two-tone analysis. .PROBE HB P(Pload)[2,-1] Calculations for Time-Domain Output In addition to a frequency-domain output, HB analysis also supports a timedomain output. The equivalent time-domain waveform is generated according to the Fourier series expansion given by Equation 33 V ( n1 )@time t = SUM OVERm ( REALV ( n1 ) [ m ] ) • cos "" ( Ω[ m ] • t ) – IMAG(V ( n1 ) [ m ] sin Ω[ m • t ] • t Where m starts from 0 to the number of frequency points in the HB simulation. The output syntax is .PRINT [HBTRAN | HBTR] V(n1) .PROBE [HBTRAN | HBTR] V(n1) The output time ranges from 0 to twice the period of the smallest frequency in the HB spectra. HSPICE® RF User Guide Z-2007.03 211 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis Output Examples .PRINT HB P(rload) .PROBE .PRINT .PROBE .PRINT .PROBE $ RMS power (spectrum) $ dissipated at the rload resistor HB V(n1,v2) $ Differential voltage (spectrum) $ between the n1,n2 nodes HB VP(out)[1] $ Phase of voltage at the out $ node, at the fundamental $ frequency HB P(Pout)[2,-1] $ RMS power delivered to the Pout $ port, at third-order intermod HBTRAN V(n1) $ Voltage at n1 in time domain HBTRAN V(n1<,n2>) $ Differential voltages between n1 $ and n2 node in time domain. Using .MEASURE with .HB Analyses ■ For transient analysis (TRAN), the independent variable for calculating .MEASURE is time. ■ For AC analysis, the independent variable for calculating .MEASURE is frequency. ■ However, as with DC analysis, the use of a .MEASURE command is peculiar for HB analysis, because it has no obvious independent variable. In HSPICE RF, the independent variable for HB .MEASURE analysis is the first swept variable specified in the .HB simulation control statement. This variable can be anything: frequency, power, voltage, current, a component value, and so on. Example 1 For the following .HB simulation control statement, the independent variable is the swept tone frequency, and the .MEASURE command values return results based on this frequency sweep: 212 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis Harmonic Balance Analysis * HARMONIC BALANCE tone-frequency sweep for amplifier .param freq1=1.91e9 power=1e-3 .HB tones=freq1 nharms=10 sweep freq1 LIN 10 1.91e9 2.0e9 .MEASURE HB Patf0 FIND P(Rload)[1] AT=1.95e9 $ Power at + f0=1.95Ghz .MEASURE HB Frq1W WHEN P(Rload)[1]=1. $ freq1 @ 1 Watt .MEASURE HB BW1W TRIG AT=1.92e9 TARG P(Rload)[1] VAL=1. + CROSS=2 $ 1 Watt bandwidth .MEASURE HB MaxPwr MAX P(Rload)[1] FROM=1.91e9 TO=2.0e9 + $ Finds max output power .MEASURE HB MinPwr MIN P(Rload)[1] FROM=1.91e9 TO=2.0e9 + $ Finds min output power Example 2 In the following example, the independent variable is the power variable, and the .MEASURE values return results based on the power sweep. Units are in Watts. * HARMONIC BALANCE power sweep for amplifier .param freq1=1.91e9 power=1e-3 .HB tones=freq1 nharms=10 sweep power DEC 10 1e-6 1e-3 .MEASURE HB Pat1uW FIND P(Rload)[1] AT=1e-6 $ Pout at 1uW .MEASURE HB Pin1W WHEN P(Rload)[1]=1. $ Pin @ 1 Watt Pout .MEASURE HB Prange1W TRIG AT=1.92e9 TARG P(Rload)[1] VAL=1. + CROSS=2 $ 1W oper. range .MEASURE HB ssGain DERIV P(Rload)[1] AT=1e-5 + $ relative power gain at 10uW input .MEASURE HB Gain3rd DERIV P(Rload)[3] AT=1e-5 + $ 3rd harmonic gain at 10uW input .MEASURE HB PAE1W FIND ‘(P(Rload)[1]-power)/P(Vdc)[0]’ + WHEN P(Rload)[1]=1 $ PAE at 1 Watt output Example 3 In this example, the independent variable is again the power variable, and the .MEASURE values return results based on the power sweep. This is a twotone sweep, where both input frequency sources are at the same power level in Watts. HSPICE® RF User Guide Z-2007.03 213 Chapter 7: Steady-State Harmonic Balance Analysis HB Output Data Files * HARMONIC BALANCE two-tone sweep for amplifier * An IP3 calculation is made at 10uW in the sweep .param freq1=1.91e9 freq2=1.91e9 power=1e-3 .HB tones=freq1,freq2 nharms=6,6 sweep power DEC 10 1e-6 1e-3 .MEASURE HB Pf1dBm FIND ’10.*LOG(P(Rload)[1,0]/1.e-3)’ + AT=1e-5 $ P(f1) at 10uW input .MEASURE HB P2f1_f2dBm FIND ’10.*LOG(P(Rload)[2,-1]/1.e-3)’ + AT=1e-5 $ P(2f1-f2) at 10uW input .MEASURE HB OIP3dBm PARAM = ‘0.5*(3.*Pf1dBm-P2f1_f2dBm)’ .MEASURE HB IIP3dBm PARAM = ‘OIP3dBm-Pf1dBm+20.0’ .MEASURE HB AM2PM DERIV VP(outp,outn)[1] AT=1e-5 + $ AM to PM Conversion in Deg/Watt If you do not specify an HB sweep, then .MEASURE assumes a single-valued independent variable sweep. You can apply the measurements to current, voltage, and power waveforms. The independent variable for measurements is the swept variable (such as power), not the frequency axis corresponding to a single HB steady state point. HSPICE RF also supports the .MEASURE [HBTRAN | HBTR] ... syntax. Similar to the .PROBE and .PRINT HBTR statements in the section Calculations for Time-Domain Output on page 211, a .MEASURE HBTR statement is applied on the signals obtained in the same way. Moreover, like a .MEASURE statement in transient analysis, the independent variable in a .MEASURE HBTR statement is time. HSPICE RF optimization can read the data from .MEASURE HB and .MEASURE HBTR statements. The optimization syntax in HSPICE RF is identical to that in the HSPICE (for details, see Statistical Analysis and Optimization in the HSPICE Simulation and Analysis User Guide). Due to the difference in the independent variable between the .MEASURE HB and .MEASURE HBTR statements, these two types of measurements cannot be mixed in a HSPICE RF optimization. But a .MEASURE HBTR statement can be combined with a .MEASURE PHASENOISE statement (see Measuring PHASENOISE Analyses with .MEASURE on page 243) and a .MEASURE HBNOISE statement (see Measuring HBNOISE Analyses with .MEASURE on page 273) in a HSPICE RF optimization flow. HB Output Data Files The results of an HB analysis are complex spectral components at each frequency point. The a[i] is the real part, and b[i] is the imaginary part of the 214 HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis HB Output Data Files complex voltage at frequency index i. The conversion to a steady state timedomain is then given by the Fourier series expansion. An HB analysis produces these output data files: ■ Output from the .PRINT HB statement is written to a .printhb# file. • The header contains the large signal fundamental frequencies. • The columns of data are labeled as HERTZ, followed by frequency indices, and then the output variable names. • The sum of the frequency indices, multiplied by the corresponding fundamental frequencies, add up to the frequency in the first column. ■ Output from the .PROBE HB statement is written to a .hb# file. It is in the same format as the HSPICE transient analysis .tr# file. Besides the output waveform, it contains the information of harmonic indices and basic tone frequencies. ■ Output from the .PRINT HBTRAN statement is written to a .printhr# file. The format is identical to a .print# file. ■ Output from the .PROBE HBTRAN statement is written to a .hr# file. The format is identical to a .tr# file. ■ Reported performance log statistics are written to a .lis file: • Name of HB data file. • Simulation time: DC operating point (op) time HB time Total simulation time • Memory used • Size of matrix (nodes * harmonics) • Final HB residual error HSPICE® RF User Guide Z-2007.03 215 Chapter 7: Steady-State Harmonic Balance Analysis HB Output Data Files Errors and Warnings Table 17 lists the errors messages and Table 18 on page 217 lists the warning messages. Table 17 216 HB Analysis Error Messages File Description HB_ERR.1 Harmonic numbers must be positive non-zero. HB_ERR.2 No .hb frequencies given. HB_ERR.3 Negative frequency given. HB_ERR.4 Number of harmonics should be greater than zero. HB_ERR.5 Different number of tones, nharms. HB_ERR.6 Bad probe node format for oscillator analysis. HB_ERR.7 Bad format for FSPTS. HB_ERR.8 Bad .hb keyword. HB_ERR.9 Tones must be specified for .hb analysis. HB_ERR.10 Nharms or intmodmax must be specified for .hb analysis. HB_ERR.11 Source harmonic out of range. HB_ERR.12 Source named in the tones list is not defined. HB_ERR.13 Source named in the tones list does not have TRANFORHB specified. HB_ERR.14 Source named in the tones list has no transient description. HB_ERR.15 Source named in the tones list must be HB, SIN, PULSE, PWL, or VMRF. HB_ERR.16 Tone specification for the source is inconsistent with its frequency. HB_ERR.17 HB oscillator analysis has reached the NULL solution. HSPICE® RF User Guide Z-2007.03 Chapter 7: Steady-State Harmonic Balance Analysis HB Output Data Files Table 17 HB Analysis Error Messages (Continued) File Description HB_ERR.18 Bad subharms format. HB_ERR.19 Modtone may not be set to the same value as tone. Table 18 HB Analysis Warning Messages File Description HB_WARN.1 .hb multiply defined. Last one will be used. HB_WARN.2 Tone specified for V/I source not specified in .HB command. HB_WARN.3 HB convergence not achieved. HB_WARN.4 Source specifies both HB and transient description. HB description will be used. HB_WARN.5 Source specifies exponential decay. HB will ignore it. HB_WARN.6 Source specifies a non-positive frequency. HB_WARN.7 Source does not fit the HB spectrum. HB_WARN.8 Source cannot be used with the TRANFORHB option. HB_WARN.9 Frequency not found from transient analysis HB_WARN.10 .hb/.hbosc will be ignored due to .env/.envosc. HB_WARN.11 HBTRANINIT does not support more than one input tone. HSPICE® RF User Guide Z-2007.03 217 Chapter 7: Steady-State Harmonic Balance Analysis References References [1] S. Maas, Nonlinear Microwave Circuits, Chapter 3, IEEE Press, 1997. [2] R. Gilmore and M.B. Steer, “Nonlinear Circuit Analysis Using the Method of Harmonic Balance - A Review of the Art, Part I, Introductory Concepts.” International Journal of Microwave and Millimeter-wave Computer-Aided Engineering, Volume 1, No. 1, pages 22-37, 1991. [3] R. Gilmore and M.B. Steer, “Nonlinear Circuit Analysis Using the Method of Harmonic Balance - A Review of the Art. Part II. Advanced Concepts.” International Journal of Microwave and Millimeter-wave Computer-Aided Engineering, Volume 1, No. 2, pages 159-180, 1991. [4] V. Rizzoli, F. Mastri, F. Sgallari, G. Spaletta, “Harmonic-Balance Simulation of Strongly Nonlinear Very Large-Size Microwave Circuits by Inexact Newton Methods,” MTT-S Digest, pages 1357-1360, 1996. [5] S. Skaggs, Efficient Harmonic Balance Modeling of Large Microwave Circuits, Ph.D. thesis, North Carolina State University, 1999. [6] R.S. Carson, High-Frequency Amplifiers, 2nd Edition, John Wiley & Sons, 1982 [7] S.Y. Liao, Microwave Circuit Analysis and Amplifier Design, Prentice-Hall, 1987. [8] J. Roychowdhury, D. Long, P. Feldmann, “Cyclostationary Noise Analysis of Large RF Circuits with Multitone Excitations”, IEEE JSCC, volume 33, number 3, March 1998. [9] Y. Saad, Iterative Methods for Sparse Linear Systems, PWS Publishing Company, 1995. [10] J. Roychowdhury, D. Long, and P. Feldmann, “Cyclostationary Noise Analysis of Large RF Circuits with Multitone Excitations,” IEEE Journal of Solid-State Circuits, volume 33, pages 324–336, March 1998. [11] K. Kurakawa, “Power waves and the Scattering Matrix,” IEEE Trans. Microwave Theory Tech., vol. MTT-13, pp. 194-202, March 1965. 218 HSPICE® RF User Guide Z-2007.03 8 Steady-State Shooting Newton Analysis 8 Describes HSPICE RF steady-state time domain analysis based on a Shooting-Newton algorithm. SN Steady-State Time Domain Analysis An advanced Shooting Newton (SN) algorithm provides additional performance and functionality to HSPICE RF for time-domain, steady-state analysis. Shooting-Newton adds analysis capabilities for PLL components, digital circuits/logic, such as ring oscillators, frequency dividers, phase/frequency detectors (PFDs), and for other digital logic circuits and RF components that require steady-state analysis, but operate with waveforms that are more square wave than sinusoidal. The Shooting-Newton algorithm effectively analyzes applications including: ■ Ring oscillators (see Chapter 9, Oscillator and Phase Noise Analysis) ■ Frequency dividers (prescalers) ■ Mixer conversion gain ■ Phase-frequency detectors (PFDs) ■ Mixer noise figure Functionality includes: ■ Both driven and oscillator (autonomous) analyses ■ Time Domain or Frequency analysis based on advanced Shooting Newton algorithm ■ Spectrum analysis specific to the SN analysis (see Shooting Newton with Fourier Transform (.SNFT) on page 224) HSPICE® RF User Guide Z-2007.03 219 Chapter 8: Steady-State Shooting Newton Analysis SN Analysis Syntax ■ Shooting Newton-based AC analysis (SNAC) (See Shooting Newton AC Analysis (.SNAC) on page 263) ■ Shooting Newton-based noise analysis (SNNOISE) (See Oscillator Analysis Using Shooting Newton (.SNOSC) on page 236) SN Analysis Syntax Shooting Newton provides two syntaxes. Syntax #1 is recommended when you are using/making Time Domain sources and measurements (for example, going from .TRAN to .SN). Syntax #2 effectively supports Frequency Domain sources and measurements (and should be used, for example, when going from .HB to .SN). Syntax #1 .SN TRES=<Tr> PERIOD=<T> [TRINIT=<Ti>] + [SWEEP parameter_sweep] [MAXTRINITCYCLES=<integer>] or, Syntax #2 .SN TONE=<F1> NHARMS=<N> [TRINIT=<Ti]> + [SWEEP parameter_sweep] [MAXTRINITCYCLES=<integer>] where 220 Parameter Description TRES The time resolution to be computed for the steady-state waveforms (in seconds). PERIOD The expected period T (seconds) of the steady-state waveforms. Enter an approximate value when using for oscillator analysis. The period of the steady-state waveform may be entered either as PERIOD or its reciprocal, TONE. TONE The fundamental frequency (in Hz). NHARMS Specifies the number of high-frequency harmonic components to include in the analysis. NHARMS defaults to PERIOD/TRES rounded to nearest integer. NHARMS is required to run subsequent SNAC, SNNOISE, SNXF, and PHASENOISE analyses. When using Syntax #1, NHARMS is computed automatically as NHARMS=Round(PERIOD/ TRES). HSPICE® RF User Guide Z-2007.03 Chapter 8: Steady-State Shooting Newton Analysis SN Analysis Syntax Parameter Description TRINIT This is the transient initialization time. If not specified, the transient initialization time will be equal to the period (for Syntax 1) or the reciprocal of the tone (for Syntax 2). SWEEP Specifies the parameter sweep. As in all main analyses in HSPICE RF such as .TRAN, .HB, etc., you can specify LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, MONTE, or OPTIMIZE. MAXTRINITCYCLES Stops SN stabilization simulation and frequency detection when the simulator detects that maxtrinitcycles have been reached in the oscnode signal, or when time=trinit, whichever comes first. Minimum cycles is 1. Options In addition to all .TRAN options, .SN analysis supports the following options. Option Default Description .OPTION SNMAXITER=<integer> 40 .OPTION SNACCURACY=<integer> 10 Maximum number, Shooting-Newton iterations Similar to the sim_accuracy definition in .TRAN, i.e., larger values of snaccuracy result in a more accurate solution but may require more time points. Because Shooting-Newton must store derivative information at every time point, the memory requirements may be significant if the number of time points is very large. The maximum integer value is 50. .OPTION LOADSNINIT=”filename” Loads the operating point saved at the end of SN initialization which is used as initial conditions for the ShootingNewton method. .OPTION SAVESNINIT=”filename” Saves the operating point at the end of SN initialization (sninit). HSPICE® RF User Guide Z-2007.03 221 Chapter 8: Steady-State Shooting Newton Analysis SN Analysis Output SN Analysis Output The output from .SN analysis is generated in both time and frequency domains. The time domain output variables are the same as for standard transient analysis: ■ individual nodal voltages: V(n1 [,n2]) ■ branch currents: I(Vxx) ■ element power dissipation: In(element) It is also possible to output the results from Shooting Newton analysis in terms of complex, frequency-domain output variables. This output format is activated by using the “SNFD” keyword in the output syntax. For output in the frequency domain, the syntax is identical to the Harmonic Balance output syntax: .PRINT SNFD TYPE(NODES | ELEM)[INDICES] .PROBE SNFD TYPE(NODES | ELEM)[INDICES] Parameter Description TYPE Specifies a harmonic type node or element. TYPE can be one of the following: 222 ■ Voltage type – ■ V = voltage magnitude and phase in degrees ■ VR = real component ■ VI = imaginary component ■ VM = magnitude ■ VP - Phase in degrees ■ VPD - Phase in degrees ■ VPR - Phase in radians ■ VDB - dB units ■ VDBM - dB relative to 1 mV HSPICE® RF User Guide Z-2007.03 Chapter 8: Steady-State Shooting Newton Analysis SN Analysis Output ■ Current type – ■ I = current magnitude and phase in degrees ■ IR = real component ■ II = imaginary component ■ IM = magnitude ■ IP - Phase in degrees ■ IPD - Phase in degrees ■ IPR - Phase in radians ■ IDB - dB units ■ IDBM - dB relative to 1 mV ■ Power type – P ■ Frequency type – ■ hertz[index], hertz[index1, index2, ...] You must specify the harmonic index for the hertz variable. The frequency of the specified harmonics is dumped. Parameter Description NODES | ELEM can be any of the following: ■ Voltage type – a single node name (n1), or a pair of node names, (n1,n2) ■ Current type – an element name (elemname) ■ Power type – a resistor (resistorname) or port (portname) element name ■ INDEX n1, is the harmonic index of the SNFD tone. Index is limited to the single tone associated with the SN analysis. Output Files The time domain data are output to .printsn0 and .sn0 files. Frequency domain data are output to .printsnf0 and .snf0 files. Output Format The format for time domain output is the same as standard transient analysis. For frequency domain output, the format is similar to HB. The main difference is that Shooting Newton output in the frequency domain is single tone only. The results of an SN analysis are complex spectral components at each frequency point. The a[i] is the real part, and b[i] is the imaginary part of the HSPICE® RF User Guide Z-2007.03 223 Chapter 8: Steady-State Shooting Newton Analysis Shooting Newton with Fourier Transform (.SNFT) complex voltage at frequency index i. The conversion to a steady state timedomain is then given by the Fourier series expansion. An SN analysis produces these output data files: ■ Output from the .PRINT SN statement is written to a .printsn# file. • The header contains the large signal fundamental frequencies. • The columns of data are labeled as HERTZ, followed by frequency indices, and then the output variable names. • The sum of the frequency indices, multiplied by the corresponding fundamental frequencies, add up to the frequency in the first column. ■ Output from the .PROBE SN statement is written to a .sn# file in the same format as the HSPICE transient analysis .tr# file. It contains the information of harmonic indices and basic tone frequencies plus the output waveform. ■ Reported performance log statistics are written to a .lis file: • Name of SN data file. • Simulation time: DC operating point (op) time SN time Total simulation time • Memory used • Size of matrix (nodes * harmonics) • Final SN residual error Shooting Newton with Fourier Transform (.SNFT) The .SNFT command is to the .SN analysis what .FFT is to the TRAN analysis, a means to provide spectrum analysis. Spectrum analysis represents a timedomain signal, within the frequency domain. .SNFT 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 .SNFT statement uses the internal time point values. By default, the .SNFT statement uses a second-order interpolation to obtain waveform samples, based on the number of points that you specify. 224 HSPICE® RF User Guide Z-2007.03 Chapter 8: Steady-State Shooting Newton Analysis Shooting Newton with Fourier Transform (.SNFT) You can use windowing functions to reduce the effects of waveform truncation on the spectral content. You can also use the .SNFT command to specify: ■ output format ■ frequency ■ number of harmonics ■ total harmonic distortion (THD) .SNFT Input Syntax The .SNFT command an take arguments with either alphanumeric or numerics and expressions. Syntax # 1 Alphanumeric input .SNFT <output_var> <START=value> <STOP=value> + <NP=value> <FORMAT=keyword> + <WINDOW=keyword> <ALFA=value> + <FREQ=value> <FMIN=value> <FMAX=value> Syntax #2 Numerics and expressions .SNFT <output_var> <START=param_expr1> <STOP=param_expr2> + <NP=param_expr3> <FORMAT=keyword> + <WINDOW=keyword> <ALFA=param_expr4> + <FREQ=param_expr5> <FMIN=param_expr6> <FMAX=param_expr7> HSPICE® RF User Guide Z-2007.03 225 Chapter 8: Steady-State Shooting Newton Analysis Shooting Newton with Fourier Transform (.SNFT) Arguments Argument Description output_var Can be any valid output variable, such as voltage, current, or power. START Start of the output variable waveform to analyze. Defaults to the START value in the .SN statement, which defaults to 0. FROM An alias for START in .SNFT statements. STOP End of the output variable waveform to analyze. Defaults to the TSTOP value in the .SN statement. TO An alias for STOP, in .SNFT statements. NP Number of points to use in the SNFT analysis. NP must be a power of 2. If NP is not a power of 2, HSPICE automatically adjusts it to the closest higher number that is a power of 2. The default is 1024. FORMAT Specifies the output format: ■ ■ WINDOW Specifies the window type to use: ■ ■ ■ ■ ■ ■ ■ ■ ALFA NORM= normalized magnitude (default) UNORM=unnormalized magnitude RECT=simple rectangular truncation window (default). BART=Bartlett (triangular) window. HANN=Hanning window. HAMM=Hamming window. BLACK=Blackman window. HARRIS=Blackman-Harris window. GAUSS=Gaussian window. KAISER=Kaiser-Bessel window. Parameter to use in GAUSS and KAISER windows to control the highest side-lobe level, bandwidth, and so on. 1.0 <= ALFA <= 20.0 The default is 3.0 FREQ 226 Frequency to analyze. If FREQ is non-zero, the output lists only the harmonics of this frequency, based on FMIN and FMAX. HSPICE also prints the THD for these harmonics. The default is 0.0 (Hz). HSPICE® RF User Guide Z-2007.03 Chapter 8: Steady-State Shooting Newton Analysis Shooting Newton with Fourier Transform (.SNFT) Argument Description FMIN Minimum frequency for which HSPICE prints SNFT output into the listing file. THD calculations also use this frequency. T=(STOP-START) The default is 1.0/T (Hz). FMAX Maximum frequency for which HSPICE prints SNFT output into the listing file. THD calculations also use this frequency. The default is 0.5*NP*FM IN (Hz). Example 1 .SNFT v(1) .SNFT v(1,2) np=1024 start=0.3m stop=0.5m freq=5.0k + window=kaiser alfa=2.5 .SNFT I(rload) start=0m to=2.0m fmin=100k fmax=120k + format=unorm .SNFT par(‘v(1) + v(2)’) from=0.2u stop=1.2u + window=harris Example 2 .SNFT v(1) np=1024 .SNFT v(2) np=1024 This example generates an .snft0 file for the SNFT of v(1) and an .snft1 file for the SNFT of v(2). .SN Signal Sources .SN analysis assumes that all stimuli are periodic with period T. If the circuit is driven with more than one periodic stimulus, then the frequencies must be all co-periodic and T must match the common period or some integer multiple of it. The .SN analysis only supports .tran (time-domain) periodic signal sources. (Refer to the .tran analysis for a detailed documentation on transient signal sources). .SN Reported Performance Log Statistics The following performance statistics are displayed: ■ DC operating time ■ Initial transient time (including user's time for circuit stabilization) ■ Total simulation time HSPICE® RF User Guide Z-2007.03 227 Chapter 8: Steady-State Shooting Newton Analysis Shooting Newton with Fourier Transform (.SNFT) ■ SN time ■ Total simulation time ■ Memory used ■ Final SN convergence residual error ■ The value of the computed frequency if the circuit is autonomous Errors/Warnings Error messages are displayed with convergence recommendations in cases of non-convergence within the maximum number of Shooting-Newton iterations. Error messages are displayed for software errors such as segmentation violations, and abort conditions such as: ■ unrecognized format, i.e., unrecognized V/I source ■ faulty input values, i.e., wrong sign, out of range value ■ unspecified values, i.e., unspecified tone ■ inconsistent values, i.e., non-commensurable tones ■ duplicate values, i.e., same entry, given more than one, the last one is always taken Limitations and Assumptions True distributed components (such as ideal delays or transmission lines) are not supported; components with hidden states are not supported. Example For a demonstration of using Shooting Newton analysis you can run the pdfcpGain.sp file shipped with the HSPICE RF distribution, located in the directory $<installdir>/hspicerf/examples. This example performs analysis on a D-flipflop phase frequency divider with charge pump, implemented in 50nm technology. The example is configured to measure the gain (volts per degree) of the DFF PFD and tri-state output combination. 228 HSPICE® RF User Guide Z-2007.03 9 Oscillator and Phase Noise Analysis 9 Describes how to use HSPICE RF to perform oscillator and phase noise analysis on autonomous (oscillator) circuits. Harmonic Balance or Shooting Newton for Oscillator Analysis HSPICE RF includes special analysis algorithms for finding the steady-state solution for oscillator circuits. In oscillators, there are no driving sources that set the frequencies of operation, but rather the fundamental oscillation frequency is one of the unknowns that is being solved by the simulator. HSPICE RF provides two approaches: either harmonic balance or analysis based on the Shooting Newton algorithm. The following sections are presented in this chapter: ■ Harmonic Balance Analysis for Frequency of Oscillation ■ Oscillator Analysis Using Shooting Newton (.SNOSC) ■ Phase Noise Analysis Harmonic Balance Analysis for Frequency of Oscillation Because the frequency of oscillation is not determined by the frequencies of driving sources, oscillator circuits are called autonomous. Autonomous simulation solves a slightly different set of nonlinear equations as shown in the following equation: Equation 34 F ( V, ω0 ) = I ( V, ω0 ) + ΩQ ( V, ω0 ) + Y ( ω0 )V + I s HSPICE harmonic balance analysis (.HBOSC) adds the fundamental frequency of oscillation to the list of unknown circuit quantities. To accommodate the extra unknown, the phase (or equivalently, the imaginary part) of one unknown HSPICE® RF User Guide Z-2007.03 229 Chapter 9: Oscillator and Phase Noise Analysis Input Syntax for Harmonic Balance Oscillator Analysis variable (generally a node voltage) is set to zero. The phases of all circuit quantities are relative to the phase, at this reference node. Additionally, HSPICE HB tries to avoid the “degenerate solution,” where all nonDC quantities are zero. Although this is a valid solution of the above equation (it is the correct solution, if the circuit does not oscillate), HB analysis might find this solution incorrectly, if the algorithm starts from a bad initial solution. Harmonic balance follows the technique described by Ngoya, et al, which uses an internally-applied voltage probe to find the oscillation voltage and frequency. The source resistance of this probe is a short circuit at the oscillation frequency, and an open circuit otherwise. HSPICE RF uses a two-tier Newton approach to find a non-zero probe voltage, which results in zero probe current. HSPICE HB approach uses the DC solution as a starting point for nonautonomous HB analysis. In addition to the DC solution, autonomous circuits need an accurate initial value for both the oscillation frequency and the probe voltage. HBOSC analysis calculates the small-signal admittance that the voltage probe sees over a range of frequencies in an attempt to find potential oscillation frequencies. Oscillation is likely to occur where the real part of the probe current is negative, and the imaginary part is zero. You can use the FSPTS parameter to specify the frequency search. You must also supply an initial guess for the large signal probe voltage. A value of one-half the supply voltage is often a good starting point. Input Syntax for Harmonic Balance Oscillator Analysis The input syntax for HBOSC analysis supports two different formats, depending on whether the PROBENODE location is specified using a circuit element (current source) or using the HBOSC PROBENODE parameters: Syntax #1 .HBOSC TONE=F1 + NHARMS=H1 PROBENODE=N1,N2,VP + <FSPTS=NUM, MIN, MAX> <SWEEP PARAMETER_SWEEP> <SUBHARMS=I> Syntax #2 (Uses current source to set PROBENODE) ISRC N1, N2 HBOSCVPROBE=VP .HBOSC TONE=F1 NHARMS=H1 <FSPTS=NUM, MIN, MAX> + <SWEEP PARAMETER_SWEEP> <SUBHARMS=I> 230 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Input Syntax for Harmonic Balance Oscillator Analysis Parameter Description TONE Approximate value for oscillation frequency (Hz). The search for an exact oscillation frequency begins from this value, unless you specify an FSPTS range or transient initialization (see HB Simulation of Ring Oscillators on page 233 for more information). NHARMS Number of harmonics to use for oscillator HB analysis. PROBENODE Circuit nodes that are probed for oscillation conditions. ■ N1 and N2 are the positive and negative nodes for a voltage probe inserted in the circuit to search for oscillation conditions. ■ VP is the initial probe voltage value (one-half the supply voltage is a suggested value). The phase of the probe voltage is forced to zero; all other phases are relative to the probe phase. HSPICE RF uses this probe to calculate small-signal admittance for the initial frequency estimates. It should be connected near the “heart” of the oscillator (near resonators, inside the ring of a ring oscillator, etc.). Note: The PROBENODE pins and approximate voltage value can also be set by using a zero amp current source that uses the HBOSCVPROBE keyword. HBOSCVPROBE=VP Sets PROBENODE with a current source. If a current source with HBOSCVPROBE is used, the PROBENODE syntax is not necessary. FSPTS Specifies the frequency search points that HSPICE RF uses in its initial small-signal frequency search to find an oscillation frequency. Optional, but recommended for high-Q and most LC oscillators. If the circuit is a ring oscillator, see HB Simulation of Ring Oscillators on page 233 for more information on how to use the HBTRANINIT option. ■ NUM is an integer. MIN and MAX are frequency values in units of Hz. If the FSPTS analysis finds an approximate oscillation frequency, the TONE parameter will be ignored. ■ HSPICE® RF User Guide Z-2007.03 231 Chapter 9: Oscillator and Phase Noise Analysis Input Syntax for Harmonic Balance Oscillator Analysis Parameter Description SWEEP Specifies the type of sweep. You can sweep up to three variables. You can specify either LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, OPTIMIZE, or MONTE. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ ■ ■ ■ SUBHARMS LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn DATA=dataname OPTIMIZE=OPTxxx MONTE=val Allows subharmonics in the analysis spectrum. The minimum nonDC frequency in the analysis spectrum is f/subharms, where f is the frequency of oscillation. Use this option if your oscillator circuit includes a divider or prescaler that will result in frequency terms that are subharmonics of the fundamental oscillation frequency Example 1 .HBOSC tone=900MEG nharms=9 probenode=gate,gnd,0.65 Performs an oscillator analysis, searching for frequencies in the vicinity of 900 MHz. This example uses nine harmonics with the probe inserted between the gate and gnd nodes. The probe voltage estimate is 0.65 V. Example 2 .HBOSC tone=2400MEG nharms=11 + probenode=drainP,drainN,1.0 fspts=20,2100MEG,2700MEG Performs an oscillator analysis, searching for frequencies in the vicinity of 2.4 GHz. This example uses 11 harmonics with the probe inserted between the drainP and drainN nodes. The probe voltage estimate is 1.0 V. Example 3 Another method to define the probenode information is through a zero-current source. The following two methods define an equivalent .HBOSC command: 232 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis HB Simulation of Ring Oscillators ■ Method 1: .HBOSC tone = 2.4G nharms = 10 + probenode = drainP, drainN, 1.0 + fspts = 20, 2.1G, 2.7G ■ Method 2: ISRC drainP drainN 0 HBOSCVPROBE = 1.0 .HBOSC tone = 2.4G nharms = 10 + fspts = 20, 2.1G, 2.7G In method 2, the PROBENODE information is defined by a current source in the circuit. Only one such current source is needed, and its current must be 0.0 with the HBOSC PROBENODE voltage defined through its HBOSCVPROBE property. HB Simulation of Ring Oscillators Ring oscillators require a slightly different simulation approach in HB. Since their oscillation is due to the inherent delay in the inverters of the ring, they are best modeled in the time domain and not in the frequency domain. Also, ring oscillator waveforms frequently approach square waves, which require a large number of harmonics to be described in the frequency domain. An accurate initial guess is important if they are going to be simulated accurately with HB. HSPICE RF HB oscillator analysis typically starts from the DC solution and looks for potential resonances in the linear portion of the circuit to determine the initial guess for the oscillation frequency. However, these resonances generally do not exist in ring oscillators, which do not contain many linear elements. HB analysis provides a second method of obtaining a good initial guess for the oscillation frequency, which is specifically intended for ring oscillators. Instead of starting from the results of a DC analysis, this method starts from the result of a transient analysis. This method is called Transient Initialization and also provides a good initial guess for all the voltages and currents in the circuit. HSPICE® RF User Guide Z-2007.03 233 Chapter 9: Oscillator and Phase Noise Analysis HBOSC Analysis Using Transient Initialization HBOSC Analysis Using Transient Initialization To perform an HBOSC analysis, use the following options in your HSPICE RF netlist. Table 19 HBOSC Analysis Options for Transient Initialization Option Description HBTRANINIT = <time> Tells HB to use transient analysis to initialize all state variables. <time> is when the circuit has reached (or is near) steady-state. Default = 0. HBTRANPTS = <npts> <npts> specifies the number of points per period for converting the time-domain data results from transient analysis, into the frequency domain. <npts> must be an integer greater than 0. The units are in nharms (nh). Default=4*nh. This option is relevant only if you set .OPTION HBTRANINIT. HBTRANSTEP = <stepsize> <stepsize> specifies the step size for the transient analysis. The default is 1/(4*nh*f0), where nh is the nharms value and f0 is the oscillation frequency. This option is relevant only if you set .OPTION HBTRANINIT. HBTRANFREQSEARCH = <1|0> If HBTRANFREQSEARCH=1 (default), then HB analysis calculates the oscillation frequency from the transient analysis. Otherwise, HB analysis assumes that the period is 1/f, where f is the frequency specified in the tones description. Note: You can specify either .OPTION HBTRANPTS or .OPTION HBTRANSTEP, but not both. You must also either specify the initial conditions or add a PWL or PULSE source to start the oscillator for transient analysis. This source should provide a 234 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis HBOSC Analysis Using Transient Initialization brief stimulus, and then return to zero. HB analysis effectively ignores this type of source, treating it as zero-valued. This method does the following: 1. If HBTRANFREQSEARCH=1, transient analysis runs for several periods, attempting to determine the oscillation frequency from the probe voltage signal. 2. Transient analysis continues until the time specified in HBTRANINIT. 3. Stores the values of all state variables over the last period of the transient analysis. 4. Transforms the state variables to the frequency domain by using a Fast Fourier Transform (FFT) to establish an initial guess for HB oscillator analysis. 5. Starts the standard HB oscillator analysis. Additional .HBOSC Analysis Options Oscillator analysis will make use of all standard HB analysis options as listed in the following table. In addition, the following options are specifically for oscillator applications. Table 20 HBOSC Analysis Options for Oscillator Applications Parameter Description HBFREQABSTOL An additional convergence criterion for oscillator analysis. HBFREQABSTOL is the maximum absolute change in frequency between solver iterations for convergence. Default is 1 Hz. HBFREQRELTOL An additional convergence criterion for oscillator analysis. HBFREQRELTOL is the maximum relative change in frequency between solver iterations for convergence. Default is 1.e-9. HBPROBETOL HBOSC analysis tries to find a probe voltage at which the probe current is less than HBPROBETOL. This option defaults to the value of HBTOL, which defaults to 1.e-9. HBMAXOSCITER Maximum number of outer-loop iterations for HBOSC analysis. It defaults to 10000. HSPICE® RF User Guide Z-2007.03 235 Chapter 9: Oscillator and Phase Noise Analysis Oscillator Analysis Using Shooting Newton (.SNOSC) .HBOSC Output Syntax The output syntax for .HBOSC analysis is identical to that for HB analysis (see Chapter 7, Steady-State Harmonic Balance Analysis). To output the final frequency of oscillation, use the HERTZ keyword. For example, hertz[1] identifies the fundamental frequency of oscillation. Oscillator Analysis Using Shooting Newton (.SNOSC) The analysis described in Chapter 8, Steady-State Shooting Newton Analysis also provides a very effective means for finding the steady-state for oscillator circuits. This approach is also very effective for ring oscillator circuits, and oscillators that operate with piecewise linear waveforms (HBOSC is superior for sinusoidal waveforms). As with the Harmonic Balance approach, the goal is to solve for the additional unknown oscillation frequency. This is accomplished in Shooting Newton by considering the period of the waveform as an additional unknown, and solving the boundary conditions at the waveform endpoints that coincide with steady-state operation. As with regular Shooting Newton analysis, input may be specified in terms of time or frequency values. .SNOSC TONE=F1 NHARMS=H1 [TRINIT=Ti] OSCNODE=N1 +[MAXTRINITCYCLES=N][SWEEP PARAMETER_SWEEP] or .SNOSC TRES=Tr PERIOD=Tp [TRINIT=Tr] OSCNODE=N1 +[MAXTRINITCYCLES=I] SWEEP PARAMETER_SWEEP 236 Parameter Description TONE Approximate value for oscillation frequency (Hz). The search for an exact oscillation frequency begins from this value. NHARMS Number of harmonics to be used for oscillator SN analysis. OSCNODE Node used to probe for oscillation conditions. This node is automatically analyzed to search for periodic behavior near the TONE or PERIOD value specified. HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Oscillator Analysis Using Shooting Newton (.SNOSC) Parameter Description TRINIT This the transient initialization time. If not specified, the transient initialization time will be equal to the period (for Syntax 1) or the reciprocal of the tone (for Syntax 2). For oscillators, we recommend specifying a transient initialization time since the default initialization time is usually too short to effectively stabilize the circuit. MAXTRINITCYCLES Stops SN stabilization simulation and frequency detection when the simulator detects that MAXTRINITCYCLES have been reached in the oscnode signal, or when time=trinit, whichever comes first. Minimum cycles is 1. The MAXTRINITCYCLES parmaeter is optional. TRES TRES is the time resolution to be computed for the steadystate waveforms (in seconds). The period of the steady-state waveform may be entered either as PERIOD or its reciprocal, TONE. PERIOD PERIOD is the expected period T (seconds) of the steadystate waveforms. Enter an approximate value when using for oscillator analysis. SWEEP Specifies the type of sweep. You can sweep up to three variables. You can specify either LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, OPTIMIZE, or MONTE. SWEEP is an optional parameter. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ ■ ■ ■ LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn DATA=dataname OPTIMIZE=OPTxxx MONTE=val Example 1 .SNOSC tone=900Meg nharms=9 trinit=10n oscnode=gate Performs an oscillator analysis, searching for periodic behavior after an initial transient analysis of 10 ns. This example uses nine harmonics while searching for an oscillation at the gate node. HSPICE® RF User Guide Z-2007.03 237 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis Example 2 .SNOSC tone=2400MEG nharms=11 trinit=20n oscnode=drainP Performs an oscillator analysis, searching for frequencies in the vicinity of 2.4 Ghz. This example uses 11 harmonics and a search at the drainP. Phase Noise Analysis Phase Noise analysis requires first running either harmonic balance (HBOSC) or Shooting Newton (SNOSC) analysis, and then PHASENOISE analysis. The PHASENOISE analysis itself is identical whether you run SNOSC or HBOSC. Figure 22 shows a simple free-running oscillator, which includes a port with injected current. Figure 22 Oscillator with Injected Current + in v(t) - An ideal oscillator would be insensitive to perturbations with a fixed amplitude, frequency, and phase represented by: Equation 35 v ( t ) = A cos [ ω0 t + φ0 ] A noisy oscillator has amplitude and phase fluctuations we can write as: Equation 36 v ( t ) = A ( t ) cos [ ω0 t + φ( t ) ] In the preceding equation: ■ A(t) is the time varying amplitude for the noisy oscillator. ■ φ( t ) is the time varying phase for the noisy oscillator. ■ ω0 is the frequency of oscillation. In most applications, the phase noise is of particular interest, because it represents frequency fluctuations about the fundamental, which you cannot 238 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis remove. These fluctuations are random processes, and are typically expressed in terms of their power spectral density. For most oscillators, the phase noise is a low-frequency modulation that creates sidebands in the oscillator’s spectrum, about ω0 . For example, the following equation represents a simple sinusoidal variation in the phase: Equation 37 v ( t ) = A cos ω0 t + θ P sin ωm t ■ θ P is the peak phase deviation, specified as θ P = Δω ⁄ ωm ■ Δω is the peak angular frequency deviation. For θ P « 1 , the following equation approximates the output: Equation 38 θP ⎧ ⎫ ----v ( t ) = A ⎨ cos ( ω0 t ) – - [ cos ( ω0 + ωP )t – cos ( ω0 – ωm )t ] ⎬ 2 ⎩ ⎭ That is, when the peak phase deviation is small, the result is frequency components on each side of the fundamental with amplitude θ P ⁄ 2 . β = θ P ,. The Single-Sideband Phase Noise L(fm) is the ratio of noise power to carrier power in a 1Hz bandwidth, at offset ωm = 2πf m , which in this case can be written as: 2 V sb 2 θ P2 θ rms ⎛ ⎞ Equation 39 L ( f m ) = -------= ------ = -----------⎝ A ⎠ 4 2 This model for oscillator noise shows that sidebands about the fundamental, due to noise, are directly related to the spectrum of the phase fluctuations θ ( t ) . The more general definition of phase noise relates it to the spectral density of phase fluctuations, i.e., θ P2 Equation 40 S φ( ωm ) = ------ = 2L ( f m ) 2 HSPICE RF uses several sophisticated analysis algorithms to predict the power spectrum for the phase variations, from which to compute phase noise. HSPICE RF uses several sophisticated analysis techniques for computing the HSPICE® RF User Guide Z-2007.03 239 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis power spectrum of the phase variations to yield the phase noise response. This information can be used to predict the spectrum of the oscillator about the fundamental frequency, and also used to predict its random jitter characteristics. PHASENOISE Input Syntax .PHASENOISE <output> <frequency_sweep> <method=0|1|2> + <carrierindex=int> <listfreq=(frequencies|none|all)> + <listcount=val> <listfloor=val> <listsources=on|off> Parameter Description output An output node, pair of nodes, or 2-terminal element. HSPICE RF references phase noise calculations to this node (or pair of nodes). Specify a pair of nodes as V(n+,n-). If you specify only one node, V(n+), then HSPICE RF assumes that the second node is ground. You can also specify a 2-terminal element. frequency_sweep A sweep of type LIN, OCT, DEC, POI, or SWEEPBLOCK. Specify the type, nsteps, and start and stop time for each sweep type, where: ■ type = Frequency sweep type, such as OCT, DEC, or LIN. nsteps = Number of steps per decade or total number of steps. ■ start = Starting frequency. ■ stop = Ending frequency. The four parameters determine the offset frequency sweep about the carrier used for the phase noise analysis. ■ LIN type nsteps start stopOCT type nsteps start stopDEC type nsteps start stopPOI type nsteps start stopSWEEPBLOCK freq1 freq2 ... freqn method 240 ■ METHOD=0 (default) selects the Nonlinear Perturbation (NLP) algorithm, which is used for low-offset frequencies. ■ METHOD=1 selects the Periodic AC (PAC) algorithm, which is used for high-offset frequencies. ■ METHOD=2 selects the Broadband Phase Noise (BPN) algorithm, which you can use to span low and high offset frequencies. You can use METHOD to specify any single method. See the section on Phasenoise Algorithms below for a more detailed discussion on using the METHOD parameter. HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis Parameter Description carrierindex Optional. Specifies the harmonic index of the carrier at which HSPICE RF computes the phase noise. The phase noise output is normalized to this carrier harmonic. Default=1. listfreq Dumps the element phase noise value to the .lis file. You can specify which frequencies the element phase noise value dumps. The frequencies must match the sweep_frequency values defined in the parameter_sweep, otherwise they are ignored. In the element phase noise output, the elements that contribute the largest phase noise are dumped first. The frequency values can be specified with the NONE or ALL keyword, which either dumps no frequencies or every frequency defined in the parameter_sweep. Frequency values must be enclosed in parentheses. For example: listfreq=(none) listfreq=(all) listfreq=(1.0G) listfreq=(1.0G, 2.0G) The default value is the first frequency value. listcount Dumps the element phase noise value to the .lis file, which is sorted from the largest to smallest value. You do not need to dump every noise element; instead, you can define listcount to dump the number of element phase-noise frequencies. For example, listcount=5 means that only the top 5 noise contributors are dumped. The default value is 20. listfloor Dumps the element phase noise value to the .lis file and defines a minimum meaningful noise value (in dBc/Hz units). Only those elements with phase-noise values larger than the listfloor value are dumped. For example, listfloor=-200 means that all noise values below -200 (dBc/Hz) are not dumped. The default value is -300 dBc/Hz. listsources Dumps the element phase-noise value to the .lis file. When the element has multiple noise sources, such as a level 54 MOSFET, which contains the thermal, shot, and 1/f noise sources. When dumping the element phase-noise value, you can decide if you need to dump the contribution from each noise source. You can specify either ON or OFF: ON dumps the contribution from each noise source and OFF does not. The default value is OFF. HSPICE® RF User Guide Z-2007.03 241 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis Phase Noise Algorithms HSPICE RF provides three algorithms for oscillator phasenoise: nonlinear perturbation, periodic AC, and broadband calculations. These algorithms are selected by setting the METHOD parameter to 0, 1, or 2, respectively. Each algorithm has their regions of validity and computational efficiency, so some thought is necessary to obtain meaningful results from a PHASENOISE simulation. For each algorithm, the region of validity depends on the particular circuit being simulated. However, there are some general rules that can be applied to oscillator types (that is, ring or harmonic) so that a valid region can be identified. And there are techniques that can be used to check validity of your simulation results. Nonlinear Perturbation Algorithm The nonlinear perturbation (NLP) algorithm, which is the default selection, is typically the fastest computation, but is valid only in a region close to the carrier. Generally, you will want to use this algorithm if you interested in phasenoise close to the carrier and do not need to determine a noise floor. NLP computation time is almost independent of the number of frequency points in the phasenoise frequency sweep. Periodic AC Algorithm The periodic AC (PAC) algorithm is valid in a region away from the carrier and is slower than the NLP algorithm. The PAC algorithm is used for getting phasenoise in the far carrier region and when you need to determine a noise floor. The computation time for the PAC algorithm is approximately linearly dependent on the number of frequency points in the phasenoise frequency sweep. If you are using the PAC algorithm, you should try to minimize the number of points in the sweep. Another issue is that the PAC algorithm becomes more ill-conditioned as you approach the carrier. This means that you may have to generate a steady-state solution with more harmonics to get an accurate simulation as you get closer to the carrier. So, if you find that the PAC is rolling off at close-in frequencies, you should rerun HB analysis with a larger number of harmonics. Although, typically, you will not see improvements in PAC accuracy beyond more than about 100-200 harmonics. 242 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis Early in your testing, the best way to verify that NLP and PAC are giving accurate results is to run both algorithms over a broad frequency range and check that the curves have some range in frequency where they overlap. Typically, you will see the NLP curve rolling off at 20 to 30 dB/decade as frequency increases, characteristic of white noise or 1/f noise behavior. Also, the PAC curve will at first be flat or even noisy close to the carrier. At some point though, you will see this curve match the NLP roll-off. The lowest frequency at which the curves overlap defines the point, fPAC above which the PAC algorithm is valid. Sometimes, by increasing the number of HB harmonics, it is possible to move fPAC to lower frequencies. The highest frequency at which the curves overlap defines the point, fNLP below which the NLP algorithm is valid. A rough rule of thumb is that fPAC = fo/Q, where fo is the carrier frequency and Q is the oscillator Q-value. This implies that for high-Q oscillators, such as crystal and some harmonic oscillators, that PAC will be accurate to values quite close to the carrier. Broadband Phasenoise Algorithm The broadband phasenoise (BPN) algorithm has been added to HSPICE RF to allow phasenoise simulation over a broad frequency range. The BPN algorithm actually runs both the NLP and PAC algorithms and then connects them in the overlap region to generate a single phasenoise curve. This algorithm is ideal for verifying the NLP and PAC accuracy regions and when you require a phasenoise curve over a broad frequency range. Measuring PHASENOISE Analyses with .MEASURE The .MEASURE PHASENOISE syntax supports five types of measurements: ■ trigger-target .MEASURE PHASENOISE result TRIG trig_var VAL = trig_val + < TD =time_delay > < CROSS = c > < RISE = r > + < FALL = f > TARG ... This measurement yields the result of the frequency difference between the trigger event and the target event. ■ find-when HSPICE® RF User Guide Z-2007.03 243 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis .MEASURE PHASENOISE result FIND out_var1 + WHEN out_var2 = out_val2 <TD = time_delay > + < RISE = r > < FALL = f > < CROSS = c> .MEASURE PHASENOISE result FIND out_var1 + At = Input_Frequency_Band value The previous measurement yields the result of a variable value at a specific input frequency band (IFB) point. .MEASURE PHASENOISE result FIND out_var1 + WHEN out_var2 = out_var3 The previous measurement yields the result at the input frequency point when out_var2 == out_var3. .MEASURE PHASENOISE result WHEN out_var2 = out_var3 The previous measurement yields the input frequency point when out_var2 == out_var3. ■ average, RMS, min, max, and peak-to-peak .MEASURE PHASENOISE result <RMS> out_var + < FROM = IFB1 > < TO = IFB2 > This measurement yields the RMS of out_var from frequency IFB1 to frequency IFB2. You can replace the <RMS> with <AVG> to find the average value of out_var. Similarly, you can replace <RMS> with <MIN>, <MAX>, or <PP> to find the result of min, max, or pp. ■ integral evaluation .MEASURE PHASENOISE result INTEGRAL out_var + < FROM = IFB1 > < TO = IFB2 > This measurement integrates the out_var value from the IFB1 frequency to the IFB2 frequency. ■ derivative evaluation .MEASURE PHASENOISE result DERIVATIVE out_var AT = IFB1 This measurement finds the derivative of out_var at the IFB1 frequency point. 244 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis Note: .MEASURE PHASENOISE cannot contain an expression that uses an phasenoise variable as an argument. You also cannot use .MEASURE PHASENOISE for error measurement and expression evaluation of PHASENOISE. The HSPICE RF optimization flow can read the measured data from a .MEASURE PHASENOISE analysis. This flow can be combined in the HSPICE RF optimization routine with a .MEASURE HBTR analysis (see Using .MEASURE with .HB Analyses on page 212) and a .MEASURE HBNOISE analysis (see Measuring HBNOISE Analyses with .MEASURE on page 273). PHASENOISE Output Syntax HSPICE RF supports the output of the phase noise as well as the phase noise due to a specified element. In addition, you can output phase noise due to the specified noise source types. In addition, you can use specialized keywords to output phase noise due to the specified noise source types, as described below. Specified Element .PRINT PHASENOISE phnoise phnoise(element_name) .PROBE PHASENOISE phnoise phnoise(element_name) In this syntax, phnoise is the phase noise parameter. The .PHASENOISE statement outputs raw data to the *.pn# and *.printpn# files. HSPICE RF outputs the phnoise data in decibels, relative to the carrier signal, per hertz, across the output nodes in the .PHASENOISE statement. The data plot is a function of the offset frequency. Units are in dBc/Hz. ■ If you use the NLP algorithm (METHOD=0) default, HSPICE RF calculates only the phase noise component. ■ If you use the PAC algorithm (METHOD=1), HSPICE RF sums both the phase and amplitude noise components to show the total noise at the output. ■ If you use the BPN algorithm (METHOD=2), HSPICE RF adds both the phase and amplitude noise components together to show the total noise at the output. HSPICE RF outputs phnoise to the .pn# file if you set .OPTION POST. Element phase noise can also be analyzed through the .PRINT and .PROBE statements, which the previous syntax shows. A single phnoise keyword specifies the phase noise for the whole circuit, and the HSPICE® RF User Guide Z-2007.03 245 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis phnoise(element_name) specifies the phase-noise value of the specified element. Example 1 .HBOSC TONE=900MEG NHARMS=9 + PROBENODE=gate,gnd,0.65 .PHASENOISE V(gate,gnd) DEC 10 100 1.0e7 + METHOD=0 CARRIERINDEX=1 $use NLP algorithm This example performs an oscillator analysis, searching for frequencies in the vicinity of 900 MHz, followed by a phase noise analysis at frequency offsets from 100 Hz to 10 MHz. Example 2 .HBOSC TONE=2400MEG NHARMS=11 + PROBENODE=drainP,drainN,1.0 + FSPTS=20,2100MEG,2700MEG + SWEEP Vtune 0.0 5.0 0.2 .PHASENOISE V(drainP,drainN) DEC 10 100 1.0e7 + METHOD=0 CARRIERINDEX=1 $use NLP algorithm This example performs a VCO analysis, searching for frequencies in the vicinity of 2.4 GHz. This example uses eleven harmonics, and sweeps the VCO tuning voltage from 0 to 5 V. HSPICE RF uses the nonlinear perturbation (NLP) algorithm to perform a phase noise analysis about the fundamental frequency for each tuning voltage value. Frequency-Dependent and Frequency-Independent Sources The phnoise_fdep keyword variable will collect all frequency-dependent noise sources' contributions to the phase noise. The phnoise_findep keyword variable will collect all frequency independent noise sources' contributions. .print phasenoise phnoise_fdep .print phasenoise phnoise_findep Frequency and Bias Dependencies The four keywords below are obvious in their names. 1. The following syntax is frequency-independent and bias-dependent: .print phasenoise phnoise_cyclo Also acceptable is: .print phasenoise phnoise_cyclostationary Where: 246 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Phase Noise Analysis cyclo or cyclostationary means anything bias-dependent. 2. The following syntax is frequency-dependent and bias independent: .print phasenoise phnoise_stationary 3. The following syntax is frequency-dependent and bias-dependent: .print phasenoise phnoise_flicker 4. The following syntax is frequency-dependent and bias-dependent: .print phasenoise phnoise_cycloflicker Also acceptable is: .print phasenoise phnoise_cyclostationaryflicker The phnoise_fdep is a combination of phnoise_flicker and phnoise_cycloflicker. The phnoise_findep is a combination of phnoise_stationary and phnoise_cycloflicker. Table 21 Summary of Noise Type Dependences Noise type frrequency-dependent bias-dependent phnoise_Stationary No No phnoise_Cyclostationary No Yes phnoise_Flicker Yes No phnoise_CycloFlicker Yes Yes phnoise_Fdep is the union of phnoise_Flicker and phnoise_CycloFlicker noise types phnoise_Findep is the union of phnoise_Stationary and phnoise_CycloFlicker noise types HSPICE® RF User Guide Z-2007.03 247 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis Phase Noise Analysis Options Table 22 lists the control options specific to PHASENOISE applications. Table 22 PHASENOISE Analysis Options Parameter Description BPNMATCHTOL=val Determines the minimum required match between the NLP and PAC phase noise algorithms. An acceptable range is 0.05dB to 5dB. The default is 0.5dB. PHASENOISEKRYLOVDIM Specifies the dimension of the Krylov subspace that the Krylov solver uses. This must be an integer greater than zero. The default is 500. PHASENOISEKRYLOVITER Specifies the maximum number of Krylov iterations that the phase noise Krylov solver takes. Analysis stops when the number of iterations reaches this value. The default is 1000. PHASENOISETOL Specifies the error tolerance for the phase noise solver. This must be a real number greater than zero. The default is 1e-8. PHNOISELORENTZ=val Turns on a Lorentzian model for the phase noise analysis. ■ ■ ■ ■ val=0: uses a linear approximation to a Lorentzian model val=1 (default): applies a lorentzian model to all noise sources val=2: applies a Lorentzian model to all nonfrequency dependent noise sources val=3: Lorentzian model applied to white noise source, Gaussian model applied to flicker noise sources. Jitter Analysis HSPICE RF provides several jitter measurements. This section defines, describes, and compares the various jitter measurements in HSPICE RF. Jitter measurements are derived from the results of an HSPICE RF phase noise 248 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis analysis. The relationships between phase noise and the latest jitter measurements are presented here, and their means for calculation. The types of jitter measurements include: Timing Jitter, RMS Phase jitter, Timing jitter is a measurement of oscillator uncertainty in the time domain. For clock applications, time domain measurements are preferable, since most specifications of concern involve time domain values. Timing jitter is the standard deviation of the timing uncertainty, which is a function of the auto correlation function in the power spectrum of the phase variations. Timing Jitter is the square root of the variance (standard deviation squared) of the timing uncertainty between two clock edges separated by an interval given byτ = N ⋅ T o, where T o is the ideal clock period. It can be written as a function of the auto correlation function of the power spectrum of phase variations as: Equation 41 2 2 σTIE ( τ ) = ------[ R φ( 0 ) – R φ( τ ) ] 2 ωo where TIE is the Time Interval error. The Weiner-Khintchine Theorem [1] relates the auto correlation function to the power spectrum of phase variations as in the following equation: ∞ Equation 42 ∞ 1 jωτ R φ( τ ) = ------ ∫ S φ( ω)e dω= 2 ∫ L ( f ) cos ( 2πfτ ) df 2π –∞ –∞ where S φ( ω) is the double-sided power spectrum of phase variations, and L ( f ) is the single-sideband phase noise. The auto correlation for τ = 0 is given by ∞ Equation 43 R φ0 ≡ 2 φrms = 2 ∫ L ( f ) sin ( πfτ ) df 2 0 which defines φrms in HSPICE RF known as RMS Phase Jitter. 2 Using the identity 2 sin α = 1 – cos 2α we can then write: ∞ Equation 44 2 σTIE 8 2 L ( f ) sin ( πfτ ) df ( τ ) = ------2 ∫ ωo 0 HSPICE® RF User Guide Z-2007.03 249 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis to enable currently supported HSPICE RF jitter measurements to be written as: ∞ Equation 45 φrms = σph ⋅ ω0 = ∫ L ( f ) df “RMS Phase Jitter” 0 ∞ 2 σTIE ( τ ) = ----ω0 ∫ 2 L ( f )sin ( πfτ ) “Timing (Time Interval Error) Jitter” 0 From these definitions, several other key jitter measurements can be derived, including Period Jitter, Tracking Jitter, Long-Term Jitter, and Cycle-to-Cycle Jitter. Period Jitter is equivalent to the value for Timing Jitter for a one period interval. We therefore have: ∞ Equation 46 2 σPER = σTIE ( τ ) = ----ω0 ∫ 2 L ( f )sin ( πfτ ) “Period Phase Jitter” 0 Tracking Jitter is equivalent to the value (in units of seconds) for RMS Phase Jitter, or: ∞ Equation 47 σtr = σph φrms 1 = --------= ----- 2 ∫ L ( f )df “Tracking Jitter” ω ω0 0 0 Long-Term Jitter is equivalent to Equation 48 2 times the Tracking Jitter, i.e.: σΔT →∞ = σTIE ( τ →∞) = φrms 2 2 --------- = ----ω0 ω0 ∞ ∫ L ( f )df “Long-Term Jitter” 0 Cycle-to-Cycle Jitter is based on the difference between adjacent Period Jitter measurements. It is given by: Equation 49 σCTC = 2 2 4σPER – σTIE ( 2T 0 ) “Cycle-to-Cycle Jitter” In general, each of the above calculations must be performed carefully over limits of integration to accurately calculate jitter expressions based on the finite 250 HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis frequency limits provided for the phase noise analysis. Linear interpolation is used, but the phase noise generally follows more of a power law expansion. Jitter Input Syntax The timing jitter calculations are derived from the results of phase noise analysis. The phase noise output syntax supports the JITTER keyword as an output keyword in addition to the PHNOISE keyword. .PRINT PHASENOISE PHNOISE JITTER .PROBE PHASENOISE PHNOISE JITTER If the JITTER keyword is present, the .PHASENOISE statement also outputs the raw jitter data to *.jt0 and *.printjt0 data files. The PHNOISE data is given in units of dBc/Hz, i.e., dB relative to the carrier, per Hz, across the output nodes specified by the PHASENOISE statement. The data plot is a function of offset frequency. If the JITTER keyword is present, .PHASENOISE outputs the TIE jitter data to *.jt0 and *.printjt0 data files. These data are plotted as a function of time in units of seconds. The jitter calculations make use of some of the parameters given in the .PHASENOISE syntax (see PHASENOISE Input Syntaxfor the syntax and examples.). The timing jitter calculations make use of the phase noise frequency sweep specification. The resulting values for type, nsteps, start, and stop result in an array of frequency points given by: 0, f 1, f 2, f 3, f 4, ...f These frequency values are used for the integration calculations necessary to compute jitter. The output of timing jitter information uses a corresponding time sampling derived via: Equation 50 1 1 1 τ 0 = -----, τ 1 = -------------, ...,τ N = --fN fN – 1 f0 .MEASURE Statements to Support Jitter Analysis The jitter-specific .MEASURE statements specify the jitter keywords as follows. (For discussion of the BER parameter, see below.) .MEASURE PHASENOISE <Jname> PERJITTER phnoise HSPICE® RF User Guide Z-2007.03 251 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis + <UNITS=(sec|rad|UI)> <BER=val> .MEASURE PHASENOISE <Jname> CTCJITTER phnoise + <UNITS=(sec|rad|UI)> <BER=val> .MEASURE PHASENOISE <Jname> RMSJITTER phnoise <FROM start_frequency> <TO end_frequency> + <UNITS=(sec|rad|UI)> <BER=val> .MEASURE PHASENOISE <Jname> PHJITTER phnoise + <FROM start_frequency> <TO end_frequency> + <UNITS=(sec|rad|UI)> <BER=val> .MEASURE PHASENOISE <Jname> TRJITTER phnoise + <FROM start_frequency> <TO end_frequency> + <UNITS=(sec|rad|UI)> <BER=val> .MEASURE PHASENOISE <Jname> LTJITTER phnoise + <FROM start_frequency> <TO end_frequency> + <UNITS=(sec|rad|UI)> <BER=val> RMSJITTER, PHJITTER, and TRJITTER are synonymous measurements, all based on the calculations described related to the RMS Phase Jitter value in units of seconds given by σph = φrms ⁄ ω0 . These measurements allow control of the integration range using the FROM and TO parameters. The measurements for PERJITTER, and CTCJITTER use the full offset frequency sweep range given for the phase noise analysis to compute values (the FROM and TO parameters are ignored if entered). As given currently in HSPICE RF, the frequency intervals can be modified for these jitter calculations (if desired, although not recommended), and UNITS can be selected between seconds, radians, and Unit Intervals. The following table specifies the calculation used for units=seconds for each jitter measurement. 252 MEASURE name Calculation used (Units=sec) RMSJITTER σph = φrms ⁄ ω0 PHJITTER σph = φrms ⁄ ω0 TRJITTER σph = φrms ⁄ ω0 PERJITTER σPER LTJITTER σΔT →∞ = 2φrms ⁄ ωo HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis MEASURE name Calculation used (Units=sec) CTCJITTER σCTC Peak-to-Peak As noted in .MEASURE Statements to Support Jitter Analysis, an additional BER (Bit Error Rate) parameter is supported. This parameter allows you to convert any jitter value from an RMS value into a Peak-to-Peak value. The RMS jitter values correspond to a 1-sigma standard deviation value for the Gaussian distribution of the jitter. Peak-to-peak values represent the full span of the Gaussian distribution. Since this span is theoretically unbounded for truly random distributions, the conversion to peak-to-peak values has to be interpreted as spanning some number of sigma values. You can arrive at this number (i.e., “sigma multiplier”) by specifying a corresponding Bit Error Rate. The term “BER” corresponds to the unitless Bit Error Rate that allows for this conversion. The following table shows conversion from various BER values into a “sigma multiplier” value which corresponds to the number of sigma standard deviations in converting from RMS to peak-to-peak values: Bit Error Rate Sigma Multiplier 10-3 6.180 10-4 7.438 10-5 8.530 10-6 9.507 10-7 10.399 10-8 11.224 10-9 11.996 10-10 12.723 10-11 13.412 10-12 14.069 HSPICE® RF User Guide Z-2007.03 253 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis Bit Error Rate Sigma Multiplier 10-13 14.698 10-14 15.301 10-15 15.883 10-16 16.444 These conversions are done in accordance with the relationship: Equation 51 1--α erfc ------- = BER 2 2 2 where, erfc is the complementary error function, and α is the Sigma Multiplier. Support for peak-to-peak conversions is included for a continuous range of BER values from 10 range). – 16 ≤α ≤10 –3 (and some values extrapolated outside this Specification of the BER parameter results in the output of the Peak to Peak jitter value, and not the RMS value. Labels for the measurements show appropriate “rms” and “p-p” labels. A BER parameter set to BER=0 is equivalent to having no parameter, and only results in the RMS calculation. Errors/Warnings Error handling and recovery is exercised to capture obvious errors in input specifications. The following error checking is performed: 254 ■ Calculations are be performed if oscillator or phase noise analysis fails. ■ ERROR if L(f) > 1 over any part of the frequency sweep (non-dB form). ■ ERROR if L(f) < 0 over any part of the frequency sweep (non-dB form). ■ Error if any time or frequency samples are negative values. ■ ERROR if BER < 0 for any Jitter measurement. ■ WARNING if BER > 1 for any Jitter measurement. ■ WARNING if f0 < 10 Hz. Message: “Jitter calculations may be ineffective for offset frequencies under 10 Hz.” HSPICE® RF User Guide Z-2007.03 Chapter 9: Oscillator and Phase Noise Analysis Jitter Analysis RMS JITTER Measurement Based on the phase noise data, the syntax of the RMS JITTER measurement is provided, where word is in units of sec (seconds), rad (radiens), or UI (Unit Interval). The default is sec. .MEASURE phasenoise integralOutMag RMSJITTER phnoise + <FROM start_frequency> <TO end_frequency> <UNITS=word> Example .meas phasenoise rj RMSJITTER phnoise from 1K to 100K + units = rad The RMSJITTER is calculated as endfrequency Equation 52 rms1 = ∑ ( 2.0 ⋅ 10.0 0.1 ⋅ phasenoise ) k = startfrequency With sec units, the RMSJITTER is calculated as Equation 53 rms1 RMSJITTER = ----------------------------2.0 ⋅ π ⋅ f0 in which PI = 3.1415926 and f0 is the tone frequency of the oscillator. With rad units, the RMSJITTER is calculated as Equation 54 RMSJITTER = rms1 With UI Unit Intervals, the RMSJITTER is calculated as Equation 55 HSPICE® RF User Guide Z-2007.03 rms1 RMSJITTER = ----------------2.0 ⋅ π 255 Chapter 9: Oscillator and Phase Noise Analysis References References [1] E. Ngoya, A. Suarez, R. Sommet, R. Quere, “Steady State Analysis of Free or Forced Oscillators by Harmonic Balance and Stability Investigation of Periodic and Quasi-Periodic Regimes,” International Journal of Microwave and Millimeter-Wave Computer-Aided Engineering, Volume 5, Number 3, pages 210-223 (1995) [2] C.R. Chang, M.B. Steer, S. Martin, E. Reese, “Computer-Aided Analysis of Free-Running Microwave Oscillators,” IEEE Trans. on Microwave Theory and Techniques, Volume 39, No. 10, pages 1735-1745, October 1991. [3] G.D. Vendelin, Design of Amplifiers and Oscillators by the S-Parameter Method, John Wiley & Sons, 1982 [4] A. Demir, A. Mehrotra, J. Roychowdhury, “Phase Noise in Oscillators: A Unifying Theory and Numerical Methods for Characterization” in Proc. IEEE DAC, pages 26-31, June 1998. [5] A. Demir, A. Mehrotra, and J. Roychowdhury, “Phase Noise in Oscillators: A Unifying Theory and Numerical Methods for Characterization,” IEEE Trans. Circuits System I, Volume 47, pages 655–674, May 2000. [6] A. van der Ziel, Noise in Solid State Devices and Circuits, John Wiley & Sons, 1986. [7] A. Hajimiri, S. Limotyrakis, and T.H. Lee, “Jitter and phase noise in ring oscillators,” IEEE J. Solid-State Circuits, vol. 34, no. 6, pp. 790-804, June 1999. [8] Jitter Analysis Techniques for High Data Rates, Application Note 1432, Agilent Technologies, Feb. 2003. [9] Characterization of Clocks and Oscillators, NIST Technical Note 1337, National Institute of Standards and Technology. [10] G.V. Klimovitch, “Near-carrier oscillator spectrum due to flicker and white noise,” Proc. ISCAS 2000 (Geneva), May 2000. 256 HSPICE® RF User Guide Z-2007.03 10 Large Signal Periodic AC, Transfer Function, and Noise Analyses 10 Describes how to use both harmonic balance-based and Shooting Newtonbased AC, and transfer function analyses, as well as nonlinear, steady-state noise analysis. The following topics are presented in this section: ■ Multitone Harmonic Balance AC Analysis (.HBAC) ■ Shooting Newton AC Analysis (.SNAC) ■ Multitone Harmonic Balance Noise (.HBNOISE) ■ Shooting Newton Noise Analysis (.SNNOISE) ■ Periodic Time-Dependent Noise Analysis (.PTDNOISE) ■ Multitone Harmonic Balance Transfer Function Analysis (.HBXF) ■ Shooting Newton Transfer Function Analysis (.SNXF) Multitone Harmonic Balance AC Analysis (.HBAC) You use the .HBAC (Harmonic Balance AC) statement for analyzing linear behavior in large-signal periodic systems. The .HBAC statement uses a periodic AC (PAC) algorithm to perform linear analysis of autonomous (oscillator) or nonautonomous (driven) circuits, where the linear coefficients are modulated by a periodic, steady-state signal. Multitone HBAC analysis extends single-tone HBAC to quasi-periodic systems with more than one periodic, steady-state tone. One application of multitone HBAC is to more efficiently determine mixer conversion gain under the influence of a strong interfering signal than is possible by running a swept three-tone HB simulation. HSPICE® RF User Guide Z-2007.03 257 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance AC Analysis (.HBAC) Prerequisites and Limitations The following prerequisites and limitations apply to HBAC: ■ Requires one and only one .HBAC statement. If you use multiple .HBAC statements, HSPICE RF uses only the last .HBAC statement. ■ Requires one and only one .HB statement. ■ Supports arbitrary number of tones. ■ Requires placing the parameter sweep in the .HB statement. ■ Requires at least one HB source. ■ Requires at least one HBAC source. ■ Supports unlimited number of HB and HBAC sources. ■ The requested maximum harmonic in a .PROBE or .PRINT statement must be less than or equal to half the number of harmonics specified in harmonic balance (that is, max_harm <= num_hb_harms / 2). Input Syntax .HBAC <frequency_sweep> Parameter Description frequency_sweep Frequency sweep range for the input signal (also referred to as the input frequency band (IFB) or fin). You can specify LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ ■ LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn DATA=dataname HBAC Analysis Options The following options directly relate to a HBAC analysis and override the corresponding PAC options if specified in the netlist: 258 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance AC Analysis (.HBAC) ■ .OPTION HBACTOL, default = 1x10-8, Range = 1x10-14 to Infinity ■ .OPTION HBACKRYLOVDIM, default = 300, Range = 1 to Infinity ■ .OPTION HBACKRYLOVITR, default = 1000, Range = 1 to Infinity If these parameters are not specified, then the following conditions apply: ■ If HBACTOL > HBTOL, then HBACTOL = HBTOL ■ If HBACKRYLOVDIM < HBKRYLOVDIM, then HBACKRYLOVDIM = HBKRYLOVDIM Output Syntax This section describes the syntax for the HBAC .PRINT and .PROBE statements. These statements are similar to those used for HB analysis. .PRINT and .PROBE Statements .PRINT HB TYPE(NODES | ELEM)[INDICES] .PROBE HB TYPE(NODES | ELEM)[INDICES] HSPICE® RF User Guide Z-2007.03 259 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance AC Analysis (.HBAC) Parameter Description TYPE Specifies a harmonic type node or element. TYPE can be one of the following: ■ ■ ■ ■ NODES | ELEM NODES or ELEM can be one of the following: ■ ■ ■ ■ 260 Voltage type – V = voltage magnitude and phase in degrees VR = real component VI = imaginary component VM = magnitude VP - Phase in degrees VPD - Phase in degrees VPR - Phase in radians VDB - dB units VDBM - dB relative to 1 mV Current type – I = current magnitude and phase in degrees IR = real component II = imaginary component IM = magnitude IP - Phase in degrees IPD - Phase in degrees IPR - Phase in radians IDB - dB units IDBM - dB relative to 1 mV Power type – P Frequency type – hertz[index], hertz[index1, index2, ...] You must specify the harmonic index for the hertz variable. The frequency of the specified harmonics is dumped. Voltage type – a single node name (n1), or a pair of node names, (n1,n2) Current type – an element name (elemname) Power type – a resistor (resistorname) or port (portname) element name Frequency type – the harmonic index for the hertz variable. The frequency of the specified harmonics is dumped. HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance AC Analysis (.HBAC) Parameter Description INDICES Index to tones in the form [n1, n2, ..., nK, +/-1]. ■ nj is the index of the j-th HB tone and the .HB statement contains K tones +/-1 is the index of the HBAC tone Wildcards are not supported if this parameter is used. ■ You can transform HB data into the time domain and output by using the following syntax:.PRINT HBTRAN ov1 [ov2 ... ovN].PROBE HBTRAN ov1 [ov2 ... ovN]. See TYPE above for voltage and current type definitions. HBAC Output Data Files An HBAC analysis produces these output data files: ■ Output from the .PRINT statement is written to a .printhb# file. This data is against the IFB points. • The header contains the large-signal fundamental and the range of small-signal frequencies. • The columns of data are labeled as F(Hz), followed by the output variable names. Each variable name has the associated mixing pair value appended. All N variable names and all M mixing pair values are printed for each swept small-signal frequency value (a total of N*M for each frequency value). ■ Output from the .PROBE statement is written to a .hb# file. This data is against the IFB points. ■ Reported performance log statistics are written to a .lis file: • Number of nodes • Number of FFT points • Number of equations • Memory in use • CPU time • Maximum Krylov iterations • Maximum Krylov dimension • Target GMRES residual HSPICE® RF User Guide Z-2007.03 261 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance AC Analysis (.HBAC) • GMRES residual • Actual Krylov iterations taken • Frequency (swept input frequency values). Errors and Warnings The following error and warning messages are used when HSPICE encounters a problem with a HBAC analysis. Error Messages HBAC frequency sweep includes negative frequencies. HBAC allows only frequencies that are greater than or equal to zero. No HB statement is specified (error at parser). HBAC requires an HB statement to generate the steady-state solution. Warning Messages More than one HBAC statement (warning at parser). HSPICE RF uses only the last HBAC statement in the netlist. No HBAC sources are specified (error at parser). HBAC requires at least one HBAC source. GMRES Convergence Failure. When GMRES (Generalized Minimum Residual) reaches the maximum number of iterations and the residual is greater than the specified tolerance. The HBAC analysis generates a warning and then continue as if the data were valid. This warning reports the following information: ■ Final GMRES Residual ■ Target GMRES Residual ■ Maximum Krylov Iterations ■ Actual Krylov Iterations taken HBAC Example The following example is shipped with the HSPICE RF distribution as mix_hbac.sp and is available in directory: $<installdir>/demo/hspicerf/examples. 262 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton AC Analysis (.SNAC) * Test HBAC: ideal I,Q mixer .OPTIONS PROBE .OPTIONS POST=2 vlo lo 0 1.0 cos(1.0 0.5 1g) TRANFORHB=1 $ Periodic, Large-Signal Input rlo lo 0 1.0 rrf rf 0 1.0 $ Noise source rrf1 rf1 rf 1.0 $ Noise source g1 0 if cur='1.0*v(lo)*v(rf)' $ mixer element c1 0 if q='1.0e-9*v(lo)*v(rf)' $ mixer element rout if ifg 1.0 vctrl ifg 0 0.0 h1 out 0 vctrl 1.0 rh1 out 0 1.0 vrf rf1 0 hbac .001 0 $ Small signal source .hb tones=1.0g nharms=3 .hbac lin 1 0.8g 0.8g .print hb v(rf1) v(lo) v(out) .probe hb v(rf1) v(lo) v(out) .measure hb vout1 find v(out)[1,-1] at=0.8g .end Shooting Newton AC Analysis (.SNAC) You use the Shooting Newton AC (.SNAC ) statement for analyzing linear behavior in large-signal periodic systems. The .SNAC statement uses a periodic AC (PAC) and Shooting Newton algorithm to perform linear analysis of nonautonomous (driven) circuits, where the linear coefficients are modulated by a periodic, steady-state signal. The following section describes the periodic AC analysis based on a Shooting Newton algorithm. This functionality is similar to the Harmonic Balance (HBAC) for periodic AC analysis. Prerequisites and Limitations The following prerequisites and limitations apply to SNAC: ■ Requires one and only one .SNAC statement. If you use multiple .SNAC statements, HSPICE RF uses only the last .SNAC statement. ■ Requires one and only one .SN statement. ■ Requires placing the parameter sweep in the .SN statement. ■ Requires at least one Periodic source. HSPICE® RF User Guide Z-2007.03 263 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton AC Analysis (.SNAC) ■ Limited to simulations that can be reduced to a single tone SN analysis. ■ Supports unlimited number of sources. ■ The requested maximum harmonic in a .PROBE or .PRINT statement must be less than or equal to half the number of harmonics specified in the SN statement (that is, max_harm ≤ nharms / 2). Input Syntax .SNAC <frequency_sweep> Parameter Description frequency_sweep Frequency sweep range for the input signal (also referred to as the input frequency band (IFB) or fin). You can specify LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ ■ LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn DATA=dataname Output Syntax This section describes the syntax for the SNAC .PRINT and .PROBE statements. These statements are similar to those used for HB analysis. .PRINT and .PROBE Statements .PRINT SN TYPE(NODES | ELEM)[INDICES] .PROBE SN TYPE(NODES | ELEM)[INDICES] 264 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton AC Analysis (.SNAC) Parameter Description TYPE Specifies a harmonic type node or element. TYPE can be one of the following: ■ ■ ■ ■ NODES | ELEM Voltage type – V = voltage magnitude and phase in degrees VR = real component VI = imaginary component VM = magnitude VP - Phase in degrees VPD - Phase in degrees VPR - Phase in radians VDB - dB units VDBM - dB relative to 1 mV Current type – I = current magnitude and phase in degrees IR = real component II = imaginary component IM = magnitude IP - Phase in degrees IPD - Phase in degrees IPR - Phase in radians IDB - dB units IDBM - dB relative to 1 mV Power type – P Frequency type – hertz[index], hertz[index1, index2, ...] You must specify the harmonic index for the hertz variable. The frequency of the specified harmonics is dumped. NODES or ELEM can be one of the following: ■ ■ ■ ■ Voltage type – a single node name (n1), or a pair of node names, (n1,n2) Current type – an element name (elemname) Power type – a resistor (resistorname) or port (portname) element name Frequency type – the harmonic index for the hertz variable. The frequency of the specified harmonics is dumped. HSPICE® RF User Guide Z-2007.03 265 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton AC Analysis (.SNAC) Parameter Description INDICES Index to tones in the form [n1, +/-1]. ■ n1 is the index of the SN tone +/-1 is the index of the SNAC tone Wildcards are not supported if this parameter is used. ■ You can transform SN data into the time domain and output by using the following syntax:.PRINT SNTRAN ov1 [ov2 ... ovN]. PROBE SNTRAN ov1 [ov2 ... ovN]. See TYPE above for voltage and current type definitions. SNAC Output Data Files A SNAC analysis produces these output data files: ■ Output from the .PRINT statement is written to a .printsnac# file. ■ This data is against the IFB points. ■ The header contains the large-signal fundamental and the range of smallsignal frequencies. ■ The columns of data are labeled as F(Hz), followed by the output variable names. Each variable name has the associated mixing pair value appended. All N variable names and all M mixing pair values are printed for each swept small-signal frequency value (a total of N*M for each frequency value). ■ Output from the .PROBE statement is written to a .snac# file. Reported performance log statistics are written to a .lis file: 266 ■ Number of nodes ■ Number of FFT points ■ Number of equations ■ Memory in use ■ CPU time ■ Maximum Krylov iterations ■ Maximum Krylov dimension ■ Target GMRES residual ■ GMRES residual HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton AC Analysis (.SNAC) ■ Actual Krylov iterations taken ■ Frequency (swept input frequency values) Errors and Warnings The following error and warning messages are used when HSPICE encounters a problem with a SNAC analysis. Error Messages SNAC frequency sweep includes negative frequencies. SNAC allows only frequencies that are greater than or equal to zero. No SN statement is specified (error at parser). SNAC requires an SN statement to generate the steady-state solution. Warning Messages More than one SNAC statement (warning at parser). HSPICE RF uses only the last SNAC statement in the netlist. No SNAC sources are specified (error at parser). SNAC requires at least one SNAC source. GMRES Convergence Failure. When GMRES (Generalized Minimum Residual) reaches the maximum number of iterations and the residual is greater than the specified tolerance. The SNAC analysis generates a warning and then continue as if the data were valid. This warning reports the following information: ■ Final GMRES Residual ■ Target GMRES Residual ■ Maximum Krylov Iterations ■ Actual Krylov Iterations taken SNAC Example The following example is shipped with the HSPICE RF distribution as mix_snac.sp and is available in directory: $<installdir>/demo/hspicerf/examples. HSPICE® RF User Guide Z-2007.03 267 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) * Test SNAC: ideal I,Q mixer -rrd .OPTIONS PROBE .OPTIONS POST=2 $.OPTIONS snmaxiter=100 .OPTIONS SNACCURACY=5 vlo lo 0 1.0 cos(1.0 0.5 1g) $ Periodic, Large-Signal SN Input rlo lo 0 1.0 rrf rf 0 1.0 $ Noise source rrf1 rf1 rf 1.0 $ Noise source g1 0 if cur='1.0*v(lo)*v(rf)' $ mixer element c1 0 if q='1.0e-9*v(lo)*v(rf)' $ mixer element rout if ifg 1.0 vctrl ifg 0 0.0 h1 out 0 vctrl 1.0 rh1 out 0 1.0 vrf rf1 0 snac .001 24.0 $ Small signal for SNAC with 1-tone SN Input .sn tones=1.0g nharms=3 .snac lin 1 0.8g 0.8g .print sn v(rf1) v(lo) v(out) .print snfd v(rf1) v(lo) v(out) .print snac v(rf1) v(lo) v(out) .measure snac vout1 find v(out)[1,-1] at=0.8g .measure snac vout2 find v(out)[0,1] at=0.8g .measure snac vout3 find v(out)[1,1] at=0.8g .measure sn vlo1 find v(lo) at=0.5n .measure sn vlo2 find v(lo) at=1n .measure snfd vlo3 find v(lo)[1] at=1 .end Multitone Harmonic Balance Noise (.HBNOISE) An HBNOISE (Harmonic Balance noise) analysis simulates the noise behavior in periodic systems. It uses a Periodic AC (PAC) algorithm to perform noise analysis of nonautonomous (driven) circuits under periodic, steady-state tone conditions. This can be extended to quasi-periodic systems having more than one periodic, steady-state tone. One application for a multitone HBNOISE analysis is determining mixer noise figures under the influence of a strong interfering signal. The PAC method simulates noise assuming that the stationary noise sources and/or the transfer function from the noise source to a specific output are periodically modulated. 268 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) ■ The modulated noise source (thermal, shot, or flicker) is modeled as a cyclostationary noise source. ■ A PAC algorithm solves the modulated transfer function. ■ You can also use the HBNOISE PAC method with correlated noise sources, including the MOSFET level 9 and level 11 models, and the behavioral noise source in the G Element (Voltage Dependent Current Source). You use the .HBNOISE statement to perform a Periodic Noise Analysis. Supported Features HBNOISE supports the following features: ■ All existing HSPICE RF noise models. ■ Uses more than one single-tone, harmonic balance to generate the steadystate solution. ■ Unlimited number of HB sources (using the same tone, possibly multiple harmonics). ■ Includes stationary, cyclostationary, frequency-dependent, and correlated noise effects. ■ Swept parameter analysis. ■ Results are independent of the number of HBAC sources in the netlist. Prerequisites and Limitations The following prerequisites and limitations apply to HBNOISE: ■ Requires one .HB statement (which determines the steady-state solution). ■ Requires at least one HB source or one TRANFORHB source. ■ Requires placing the parameter sweep in the .HB statement. ■ The requested maximum harmonic in .HBNOISE must be less than or equal to half the number of harmonics used in harmonic balance (that is, max_harm <= num_hb_harms/2). Input Syntax .HBNOISE [output] [insrc] [parameter_sweep] + <[n1, n2, ..., nk,+/-1]> HSPICE® RF User Guide Z-2007.03 269 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) + <listfreq=(frequencies|none|all)> <listcount=val> + <listfloor=val> <listsources=on|off> Parameter Description output Output node, pair of nodes, or 2-terminal element. HSPICE RF references equivalent noise output to this node (or pair of nodes). Specify a pair of nodes as V(n+,n-). If you specify only one node, V(n+), then HSPICE RF assumes that the second node is ground. You can also specify a 2-terminal element name that refers to an existing element in the netlist. insrc An input source. If this is a resistor, HSPICE RF uses it as a reference noise source to determine the noise figure. If the resistance value is 0, the result is an infinite noise figure. parameter_sweep Frequency sweep range for the input signal. Also referred to as the input frequency band (IFB) or fin). You can specify LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, MONTE, or OPTIMIZE sweeps. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ n1,n2,...,nk, +/-1 LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn Index term defining the output frequency band (OFB or fout) at which the noise is evaluated. Generally, fout=ABS(n1*f+n2*f2+...+nk*fk+/-fin) Where: ■ f1,f2,...,fk are the first through k-th steady-state tones determined from the harmonic balance solution ■ fin is the IFB defined by parameter_sweep. The default index term is [1,1,...1,-1]. For a single tone analysis, the default mode is consistent with simulating a lowside, down conversion mixer where the RF signal is specified by the IFB and the noise is measured at a down-converted frequency that the OFB specifies. In general, you can use the [n1,n2,...,nk,+/-1] index term to specify an arbitrary offset. The noise figure measurement is also dependent on this index term. 270 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) Parameter Description listfreq Prints the element noise value to the .lis file. You can specify at which frequencies the element noise value is printed. The frequencies must match the sweep_frequency values defined in the parameter_sweep, otherwise they are ignored. In the element noise output, the elements that contribute the largest noise are printed first. The frequency values can be specified with the NONE or ALL keyword, which either prints no frequencies or every frequency defined in parameter_sweep. Frequency values must be enclosed in parentheses. For example:listfreq=(none) listfreq=(all) listfreq=(1.0G) listfreq=(1.0G, 2.0G)The default value is NONE. listcount Prints the element noise value to the .lis file, which is sorted from the largest to smallest value. You do not need to print every noise element; instead, you can define listcount to print the number of element noise frequencies. For example, listcount=5 means that only the top 5 noise contributors are printed. The default value is 1. listfloor Prints the element noise value to the .lis file and defines a minimum meaningful noise value (in V/Hz1/2 units). Only those elements with noise values larger than listfloor are printed. The default value is 1.0e-14 V/Hz1/2. listsources Prints the element noise value to the .lis file when the element has multiple noise sources, such as a FET, which contains the thermal, shot, and 1/f noise sources. You can specify either ON or OFF: ON Prints the contribution from each noise source and OFF does not. The default value is OFF. Output Syntax This section describes the syntax for the HBNOISE .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT HBNOISE <ONOISE> <NF> <SSNF> <DSNF> HSPICE® RF User Guide Z-2007.03 271 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) .PROBE HBNOISE <ONOISE> <NF> <SSNF> <DSNF> Parameter Description ONOISE Outputs the voltage noise at the output frequency band (OFB) across the output nodes in the .HBNOISE statement. The data is plotted as a function of the input frequency band (IFB) points. Units are in V/Hz1/2. Simulation ignores ONOISE when applied to autonomous circuits. NF SSNF NF and SSNF both output a single-side band noise figure as a function of the IFB points: NF = SSNF = 10 Log(SSF) Single side-band noise factor, SSF = {(Total Noise at output, at OFB, originating from all frequencies) - (Load Noise originating from OFB)} / (Input Source Noise originating from IFB). DSNF DSNF outputs a double side-band noise figure as a function of the IFB points. DSNF = 10 Log(DSF) Double side-band noise factor, DSF = {(Total Noise at output, at the OFB, originating from all frequencies) - (Load Noise originating from the OFB)} / (Input Source Noise originating from the IFB and from the image of IFB). Output Data Files An HBNOISE analysis produces these output data files: ■ Output from the .PRINT statement is written to a .printpn# file. ■ Output from the .PROBE statement is written to a .pn# file. Both the *.printpn# and *.pn# files output data against the input frequency band points. ■ 272 Standard output information is written to a .lis file: • simulation time • HBNOISE linear solver method • HBNOISE simulation time • total simulation time HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) Measuring HBNOISE Analyses with .MEASURE Note: A .MEASURE HBNOISE statement cannot contain an expression that uses a HBNOISE variable as an argument. Also, you cannot use a .MEASURE HBNOISE statement for error measurement and expression evaluation of HBNOISE. The .MEASURE HBNOISE syntax supports four types of measurements: ■ Find-when .MEASURE HBNOISE result FIND out_var1 + At = Input_Frequency_Band value The previous measurement yields the result of a variable value at a specific IFB point. .MEASURE HBNOISE result FIND out_var1 + WHEN out_var2 = out_var3 The previous measurement yields the result at the input frequency point when out_var2 == out_var3. .MEASURE HBNOISE result WHEN out_var2 = out_var3 The previous measurement yields the input frequency point when out_var2 == out_var3. ■ Average, RMS, min, max, and peak-to-peak .MEASURE HBNOISE result <RMS> out_var < FROM = IFB1 > + < TO = IFB2 > ■ Integral evaluation .MEASURE HBNOISE result INTEGRAL out_var + < FROM = IFB1 > < TO = IFB2 > This measurement integrates the out_var value from the IFB1 frequency to the IFB2 frequency. ■ Derivative evaluation .MEASURE HBNOISE result DERIVATIVE out_var AT = IFB1 This measurement finds the derivative of out_var at the IFB1 frequency point. HSPICE® RF User Guide Z-2007.03 273 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Noise (.HBNOISE) Note: .MEASURE HBNOISE cannot contain an expression that uses an hbnoise variable as an argument. You also cannot use .MEASURE HBNOISE for error measurement and expression evaluation of HBNOISE. The HSPICE RF optimization flow can read the measured data from a .MEASURE HBNOISE analysis. This flow can be combined in the HSPICE RF optimization routine with a .MEASURE HBTR analysis (see Using .MEASURE with .HB Analyses on page 212) and a .MEASURE PHASENOISE analysis (see Measuring PHASENOISE Analyses with .MEASURE on page 243). Errors and Warnings HBNOISE Errors See the list of HBAC Errors and Warnings on page 262. HBNOISE Example This example performs an HB analysis, then runs an HBNOISE analysis over a range of frequencies, from 9.0e8 to 9.2e8 Hz. Simulation outputs the output noise at V(out) and the single side-band noise figure versus IFB, from 1e8 to 1.2e8 Hz, to the *.pn0 file. The netlist for this example is shown immediately following. $$*-Ideal mixer + noise source $ prints total noise at the output (1.57156p V/sqrt-Hz), $ single-sideband noise figure, (3.01 dB) $ double-sideband noise figure. (0 dB) .OPTION PROBE .OPTION POST=2 vlo lo 0 0.0 hb 1.0 0 1 1$ Periodic, HB Input Ilo lo 0 0 rsrc rfin rf1 1.0$ Noise source c1 0 if q='1.0e-9*v(lo)*v(rfin)' $ mixer element g1 0 if cur=’1.0*v(lo)*v(rfin)’ $ mixer element rout if 0 1.0 vrf rf1 0 $ hbac 2.0 0.0 .hb tones=1.0g nharms=4 $ sweep mval 1 2 1 .HBNOISE rout rsrc lin 11 0.90g 0.92g .print HBNOISE onoise ssnf dsnf .probe HBNOISE onoise ssnf dsnf .end 274 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Noise Analysis (.SNNOISE) Shooting Newton Noise Analysis (.SNNOISE) A SNNOISE (Shooting Newton noise) analysis simulates the noise behavior in periodic systems. It uses a Periodic AC (PAC) algorithm to perform noise analysis of nonautonomous (driven) circuits under periodic, steady-state tone conditions. SNNOISE is similar to the HBNOISE analysis. The PAC method simulates noise assuming that the stationary noise sources and/or the transfer function from the noise source to a specific output are periodically modulated. ■ The modulated noise source (thermal, shot, or flicker) is modeled as a cyclostationary noise source. ■ A PAC algorithm solves the modulated transfer function. ■ You can also use the SNNOISE PAC method with correlated noise sources, including the MOSFET Level 9 and Level 11 models, and the behavioral noise source in the G Element (Voltage Dependent Current Source). You use the .SNNOISE statement to perform a Periodic Noise Analysis. Supported Features SNNOISE supports the following features: ■ All existing HSPICE RF noise models. ■ Uses Shooting Newton to generate the steady-state solution. ■ Unlimited number of sources. ■ Includes stationary, cyclostationary, frequency-dependent, and correlated noise effects. ■ Swept parameter analysis. ■ Results are independent of the number of SNAC sources in the netlist. Prerequisites and Limitations The following prerequisites and limitations apply to SNNOISE: ■ Requires one .SN statement (which determines the steady-state solution). ■ Requires at least one Periodic source. Does not recognize HB sources. ■ Requires placing the parameter sweep in the .SN statement. HSPICE® RF User Guide Z-2007.03 275 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Noise Analysis (.SNNOISE) Input Syntax .SNNOISE [output] [insrc] [parameter_sweep] + <[n1+/-1]> + <listfreq=(frequencies|none|all)> <listcount=val> + <listfloor=val> <listsources=on|off> Parameter Description output Output node, pair of nodes, or 2-terminal element. HSPICE RF references equivalent noise output to this node (or pair of nodes). Specify a pair of nodes as V(n+,n-). If you specify only one node, V(n+), then HSPICE RF assumes that the second node is ground. You can also specify a 2-terminal element name that refers to an existing element in the netlist. insrc An input source. If this is a resistor, HSPICE RF uses it as a reference noise source to determine the noise figure. If the resistance value is 0, the result is an infinite noise figure. parameter_sweep Frequency sweep range for the input signal. Also referred to as the input frequency band (IFB) or fin). You can specify LIN, DEC, OCT, POI, SWEEPBLOCK, DATA, MONTE, or OPTIMIZE sweeps. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ 276 LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Noise Analysis (.SNNOISE) Parameter Description n1,+/-1 Index term defining the output frequency band (OFB or fout) at which the noise is evaluated. Generally, fout=ABS(n1*f1+/-fin) Where: ■ f1 is the fundamental harmonic (tone) determined in the Shooting Newton analysis ■ n1 is the associated harmonic multiplier ■ n1,n2,...,nk are the associated harmonic multipliers; n1 can be any non-negative integer ≤ nharm defined in the .SN statement; +/-1 is fixed, either +1 or -1 ■ fin is the IFB defined by parameter_sweep. The default index term is [1,-1]. For a single tone analysis, the default mode is consistent with simulating a low-side, down conversion mixer where the RF signal is specified by the IFB and the noise is measured at a down-converted frequency that the OFB specifies. In general, you can use the [n1,+/-1] index term to specify an arbitrary offset. The noise figure measurement is also dependent on this index term. (See Measuring SNNOISE Analyses with .MEASURE below.) listfreq Prints the element noise value to the .lis file. You can specify at which frequencies the element noise value is printed. The frequencies must match the sweep_frequency values defined in the parameter_sweep, otherwise they are ignored. In the element noise output, the elements that contribute the largest noise are printed first. The frequency values can be specified with the NONE or ALL keyword, which either prints no frequencies or every frequency defined in parameter_sweep. Frequency values must be enclosed in parentheses. For example:listfreq=(none) listfreq=(all) listfreq=(1.0G) listfreq=(1.0G, 2.0G) The default value is NONE. listcount HSPICE® RF User Guide Z-2007.03 Prints the element noise value to the .lis file, which is sorted from the largest to smallest value. You do not need to print every noise element; instead, you can define listcount to print the number of element noise frequencies. For example, listcount=5 means that only the top 5 noise contributors are printed. The default value is 1. 277 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Noise Analysis (.SNNOISE) Parameter Description listfloor Prints the element noise value to the .lis file and defines a minimum meaningful noise value (in V/Hz1/2 units). Only those elements with noise values larger than listfloor are printed. The default value is 1.0e-14 V/Hz1/2. listsources Prints the element noise value to the .lis file when the element has multiple noise sources, such as a FET, which contains the thermal, shot, and 1/f noise sources. You can specify either ON or OFF: ON Prints the contribution from each noise source and OFF does not. The default value is OFF. Output Syntax This section describes the syntax for the SNNOISE .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT SNNOISE <ONOISE> <NF> <SSNF> <DSNF> .PROBE SNNOISE <ONOISE> <NF> <SSNF> <DSNF> Parameter Description ONOISE Outputs the voltage noise at the output frequency band (OFB) across the output nodes in the .SNNOISE statement. The data is plotted as a function of the input frequency band (IFB) points. Units are in V/Hz1/2. Simulation ignores ONOISE when applied to autonomous circuits. NF SSNF NF and SSNF both output a single-side band noise figure as a function of the IFB points: NF = SSNF = 10 Log(SSF) Single side-band noise factor, SSF = {(Total Noise at output, at OFB, originating from all frequencies) - (Load Noise originating from OFB)} / (Input Source Noise originating from IFB). 278 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Noise Analysis (.SNNOISE) Parameter Description DSNF DSNF outputs a double side-band noise figure as a function of the IFB points. DSNF = 10 Log(DSF) Double side-band noise factor, DSF = {(Total Noise at output, at the OFB, originating from all frequencies) - (Load Noise originating from the OFB)} / (Input Source Noise originating from the IFB and from the image of IFB). Output Data Files An SNNOISE analysis produces these output data files: ■ Output from the .PRINT statement is written to a .printsnpn# file. ■ Output from the .PROBE statement is written to a .snpn# file. Both the *.printsnpn# and *.pn# files output data against the input frequency band points. ■ Standard output information is written to a .lis file: • simulation time • SNNOISE linear solver method • SNNOISE simulation time • total simulation time Measuring SNNOISE Analyses with .MEASURE Note: A .MEASURE SNNOISE statement cannot contain an expression that uses a SNNOISE variable as an argument. Also, you cannot use a .MEASURE SNNOISE statement for error measurement and expression evaluation of SNNOISE. The .MEASURE SNNOISE syntax supports four types of measurements: ■ Find-when .MEASURE SNNOISE result FIND out_var1 + At = Input_Frequency_Band value HSPICE® RF User Guide Z-2007.03 279 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Noise Analysis (.SNNOISE) The previous measurement yields the result of a variable value at a specific IFB point. .MEASURE SNNOISE result FIND out_var1 + WHEN out_var2 = out_var3 The previous measurement yields the result at the input frequency point when out_var2 == out_var3. .MEASURE SNNOISE result WHEN out_var2 = out_var3 The previous measurement yields the input frequency point when out_var2 == out_var3. ■ Average, RMS, min, max, and peak-to-peak .MEASURE SNNOISE result <RMS> out_var < FROM = IFB1 > + < TO = IFB2 > ■ Integral evaluation .MEASURE SNNOISE result INTEGRAL out_var + < FROM = IFB1 > < TO = IFB2 > This measurement integrates the out_var value from the IFB1 frequency to the IFB2 frequency. ■ Derivative evaluation .MEASURE SNNOISE result DERIVATIVE out_var AT = IFB1 This measurement finds the derivative of out_var at the IFB1 frequency point. Note: .MEASURE SNNOISE cannot contain an expression that uses an hbnoise variable as an argument. You also cannot use .MEASURE SNNOISE for error measurement and expression evaluation of SNNOISE. SNNOISE Analysis Example This example performs an SN analysis, then runs an SNNOISE analysis over a range of frequencies, from 9.0e8 to 9.2e8 Hz. Simulation outputs the output noise at V(out) and the single side-band noise figure versus IFB, from 9.0e8 to 9.2e8 Hz, to the *.pn0 file. The netlist for this example is shown immediately following. 280 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Periodic Time-Dependent Noise Analysis (.PTDNOISE) * $$*-Ideal mixer + noise source $ prints total noise PSD at the output (2.47e-20 V^2) when q=0 $ single-sideband noise figure, (3.01 dB) $ double-sideband noise figure. (0 dB) .OPTION PROBE .OPTION POST=2 vlo lo 0 0.0 cos (0 1.0 1.0g 0 0 0) Ilo lo 0 0 rsrc rfin rf1 1.0$ Noise source g1 0 if cur='1.0*v(lo)*v(rfin)' $ mixer element c1 0 if q='1.0e-9*v(lo)*v(rfin)' $ mixer element rout if 0 1.0 vrf rf1 0 $ hbac 2.0 0.0 .option delmax=0.002n .SN tones=1G nharms=4 trstab=10n .SNNOISE rout rsrc lin 11 0.90g 0.92g .probe SNNOISE onoise ssnf dsnf .print SNNOISE onoise ssnf dsnf .end Periodic Time-Dependent Noise Analysis (.PTDNOISE) While HBNOISE and SNNOISE calculate a time-averaged power spectral density, there are applications where a characterization of the timedependence of the noise is required. These applications include computation of jitter associated with a noisy signal crossing a threshold and computation of the noise associated with discretizing an analog signal, which computes the noise in a periodically driven circuit at a point in time. Periodic Time-Dependent noise analysis (PTDNOISE) calculates the noise spectrum and the total noise at a point in time. Jitter in a digital threshold circuit can then be determined from the total noise and the digital signal slew rate. Circuits driven by large periodic signals produce cyclostationary noise, that is, the noise characteristics are periodic in time. Cyclostationary noise can be characterized in several ways, with the particular application determining which is appropriate.[9] The time-average power spectral density (PSD) ignores frequency correlations in the noise, but is adequate when the fundamental frequency of the cyclostationary noise is much larger than the bandwidth of interest. The time-average PSD is calculated in the HBNOISE/SNNOISE analyses. [10] The harmonic power spectral density (HPSD) or equivalently, the autocorrelation function, R(t1,t2), contains the correlation information between HSPICE® RF User Guide Z-2007.03 281 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Periodic Time-Dependent Noise Analysis (.PTDNOISE) noise sidebands that is necessary to build behavioral cyclostationary noise sources and to separate the amplitude modulation (AM) and phase modulation (PM) noise components. The time-dependent power spectral density (TDPSD) can be integrated over frequency to yield the time-dependent noise (TDN). TDN can then be used to determine jitter associated with a noisy signal crossing a threshold. PTDNOISE analysis allows the calculation of TDPSD, TDN, and jitter. By measuring the jitter associated with a noisy signal crossing a threshold, jitter is modeled by displacing the time in a noise free signal v(t) with a stochastic process j(t). Equation 56 V jitter ( t ) = v ( t + j ( t ) ) We can also determine the voltage at this node including the time-dependent noise n(t): Equation 57 Vn ( t ) = v ( t ) + n ( t ) by equating these two representations, expanding in a Taylor series, and dropping higher order terms, as follows: Equation 58 V ( t ) + n ( t ) = v ( t + j ( t ) ) = v ( t ) + dv ( t ) ⁄ dt ⋅ j ( t ) + … Equation 59 N ( t ) = dv ( t ) ⁄ dt ⋅ j ( t In terms of variances, jitter is then defined as: 2 Equation 60 Var ( j ( t ) ) = n ( t ) ⁄ ( dv ( t ) ⁄ dt ) PTDNOISE Input Syntax .PTDNOISE [output] [time_value] <time_delta> + [frequency_sweep] + <listfreq=(frequencies|none|all)> <listcount=val> + <listfloor=val> <listsources=on|off> 282 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Periodic Time-Dependent Noise Analysis (.PTDNOISE) Parameter Description output Can be an output node, pair of nodes, or 2-terminal element. HSPICE RF references the equivalent noise output to this node (or pair of nodes). Specify a pair of nodes as V(n+,n-). If you specify only one node, V(n+, n-). If you specify only one node, V(n+), then HSPICE RF assumes the second node is ground. You can also specify a 2-terminal element name that refers to an existing element in the netlist. time_value Time point at which time domain noise is evaluated. Specify either a time point explicitly, such as: TIME=value, where value is either numerical or a parameter name or A .MEASURE name associated with a time domain .MEASURE statement located in the netlist. PTDNOISE uses the time point generated from the .MEASURE statement to evaluate the noise characteristics. This is useful if you want to evaluate noise or jitter when a signal reaches some threshold value. time_delta A time value used to determine the slew rate of the time-domain output signal. Specified as TDELTA=value. The signal slew rate is then determined by the output signal at TIME +/- TDELTA and dividing this difference by 2 x TDELTA. This slew rate is then used in the calculation of the strobed jitter. If this term is omitted a default value of 0.01 x the .SN period is assumed. frequency_sweep Frequency sweep range for the output noise spectrum. The upper and lower limits also specify the integral range in calculating the integrated noise value. Specify LIN,DEC, OCT, POI, SWEEPBLOCK, DATA sweeps. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: LIN nsteps start stop DECnsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn HSPICE® RF User Guide Z-2007.03 283 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Periodic Time-Dependent Noise Analysis (.PTDNOISE) Parameter Description listfreq Prints the element noise value to the .lis file. This information is only printed if a noise spectrum is requested in a PRINT or PROBE statement. (See PTDNOISE Output Syntax and File Format.) You can specify which frequencies the element noise is printed. The frequencies must match the sweep_frequency values defined in the frequency_sweep, otherwise they are ignored. In the element noise output, the elements that contribute the largest noise are printed first. The frequency values can be specified with the NONE or ALL keyword, which either prints no frequencies or every frequency defined in frequency_sweep. Frequency values must be enclosed in parentheses. For example: listfreq=(none) listfreq=(all) listfreq=(1.0G) listfreq=(1.0G, 2.0G) The default value is NONE. listcount Prints the element noise value to the .lis file, which is sorted from the largest to smallest value. You do not need to print every noise element; instead, you can define listcount to print the number of element noise frequencies. For example, listcount=5 means that only the top 5 noise contributors are printed. The default value is 1. listfloor Prints the element noise value to the .lis file and defines a minimum meaningful noise value (in V/Hz1/2 units). Only those elements with noise values larger than listfloor are printed. The default value is 1.0e-14 V/Hz1/2. listsources Prints the element noise value to the .lis file when the element has multiple noise sources, such as a FET, which contains the thermal, shot, and 1/f noise sources. You can specify either ON or OFF: ON prints the contribution from each noise source and OFF does not. The default value is OFF. PTDNOISE Output Syntax and File Format PTDNOISE output syntax allows for the output of one parameter: onoise. .PROBE PTDNOISE <onoise> 284 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Periodic Time-Dependent Noise Analysis (.PTDNOISE) .PRINT PTDNOISE <onoise> Parameter Units Description onoise Noise voltage spectral density at each frequency point specified by frequency_sweep at the time point specified by time_value V⁄ Hz Output File Format The following PTDNOISE output files are generated depending on the user input: File Description *.printptn# Writes output from the .PRINT statement when using HB to obtain the steady state solution *.ptn# Writes output from the .PROBE statement when using HB to obtain the steady state solution *.printsnptn# Reports output from the .PRINT statement when using SN to obtain the steady state solution. *.snptn# Writes output from the .PROBE statement when using SN to obtain the steady state solution. *.lis Standard output file *.lis contains the following information: Performance Statistics Log Number of Nodes Number of FFT Points Number of Equations Memory in use Maximum Krylov iterations Maximum Krylov Dimension Target GMRES Residual Gmres Residual Actual Krylov Iterations taken Frequency (swept input frequency values) HSPICE® RF User Guide Z-2007.03 285 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Periodic Time-Dependent Noise Analysis (.PTDNOISE) File Description Noise source contributions are listed sequentially and are controlled by the PTDNOISE command line parameters: listtime, listfreq, listcount, listfloor, and listsources. .MEASURE Syntax and File Format The syntax for .MEASURE PTDNOISE is: .MEASURE PTDNOISE meas_name STROBEJITTER onoise freq_sweep Only STROBEJITTER can be specified. However, this will result in all of the parameters listed below, being output to the *.msnptn# file. .MEASURE PTDNOISE allows for the measurement of these parameters: integnoise, time-point, tdelta-value, slewrate, and strobed jitter. Parameter Units Description strobejitter sec Calculated from the noise voltage (integrated over the frequency range specified by frequency_range), divided by the slewrate at the same node(s), at the time point specified by time_value. While only STROBEJITTER can be specified, all of the parameters listed below, are also output to the *.msnptn# file. 286 integptdnoise V Total ptd voltage noise in V2 ⁄ ( Hz )(integrated over a frequency range specified by frequency_range) at the time point specified by time_value. The value is stated as a voltage (V). timepoint sec Time point at which the ptdnoise and slewrate are calculated. tdelta-value sec TDELTA value used to calculate slewrate. slewrate v/sec Output signal slewrate at the time point specified by time_value. HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Transfer Function Analysis (.HBXF) Measure File Format File Description *.msnptn# Writes output from the .MEASURE statement when using SN to obtain the steady state solution. Error Handling and Warnings Error messages are generated under the following circumstances: ■ PTDNOISE frequency sweep includes negative frequencies. PTDNOISE allows only frequencies that are greater than or equal to zero. ■ PTDNOISE time sweep includes negative times. PTDNOISE allows only time points that are greater than or equal to zero. ■ No SN statement is specified (error at parser). PTDNOISE requires an SN statement to generate the steady-state solution. ■ Incorrect match to .MEASURE statement. A warning is issued for a PTDNOISE convergence failure. When the gmres solver reaches the maximum number of iterations and the residual is greater than the specified tolerance, PTDNOISE generates a warning and then continue as if the data were valid. The Warning reports the following information: Final GMRES Residual Target GMRES Residual Maximum Krylov Iterations Actual Krylov Iterations taken Multitone Harmonic Balance Transfer Function Analysis (.HBXF) The .HBXF command calculates the transfer function from a given source in the circuit to a designated output. Frequency conversion is calculated from the input frequencies to a single output frequency that is specified with the command. The relationship between the .HBXF command and the input/output is expressed in the following equation: HSPICE® RF User Guide Z-2007.03 287 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Transfer Function Analysis (.HBXF) Equation 61 Y m ( jω0 ) = ∑ HBXFm,n ( jω0 ,j ( ω + Δω) ) ⋅ X n ( j ( ω + Δω) ) ωε W Where: ■ HBXF m ,n ( jω0 ,j ( ω + Δω) ) is the transfer function from input port n to the output port m ■ W is the set of all possible harmonics ■ ω + Δω is the input frequency ■ Δω is the offset frequency ■ m is the output node number ■ n is the input node number ■ ω0 is the output frequency ■ Y is the output (voltage or current) ■ X is the input (voltage or current) Supported Features The .HBXF command supports the following features: ■ All existing HSPICE RF models and elements ■ Sweep parameter analysis ■ Unlimited number of HB sources Prerequisites and Limitations The following prerequisites and limitations apply to the .HBXF command: 288 ■ Only one .HBXF statement is required. If you use multiple .HBXF statements, HSPICE RF only uses the last .HBXF statement. ■ At least one .HB statement is required, which determines the steady-state solution. ■ Parameter sweeps must be placed in .HB statements. HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Transfer Function Analysis (.HBXF) Input Syntax .HBXF out_var <freq_sweep> Parameter Description out_var Specify i(2_port_elem) or V(n1<,n2>) freq_sweep Frequency sweep range for the input signal (also referred to as the input frequency band (IFB or fin)). A sweep of type LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ LIN nsteps start stop DEC nsteps start stop ■ OCT nsteps start stop ■ POI nsteps freq_values ■ SWEEPBLOCK = BlockName Specify the frequency sweep range for the output signal. HSPICE RF determines the offset frequency in the input sidebands; for example, ■ f1 = abs(fout - k*f0) s.t. f1<=f0/2 The f0 is the steady-state fundamental tone, and f1 is the input frequency. Output Syntax This section describes the syntax for the HBXF .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT HBXF TYPE(NODES | ELEM) HSPICE® RF User Guide Z-2007.03 289 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Multitone Harmonic Balance Transfer Function Analysis (.HBXF) .PROBE HBXF TYPE(NODES | ELEM) Parameter Description TYPE TYPE can be one of the following: ■ TFV = existing source TFI = placeholder value for the current source attached to the given node. The transfer function is computed on the output variables and input current or voltage. ■ NODES | ELEM NODES or ELEM can be one of the following: ■ ■ ■ Voltage type – a single node name (n1), or a pair of node names, (n1,n2) Current type – an element name (elemname) Power type – a resistor (resistorname) or port (portname) element name. Output Data Files An HBXF calculation produces these output data files: ■ Output from the .PRINT statement is written to a .printxf# file. • The output is in ohms, siemens, or undesignated units, and the header in the output file is Z(..). Y(..) or GAIN(..). ■ Output from the .PROBE statement is written to a .xf# file. ■ Reported performance log statistics are written to a .lis file: • HBXF CPU time • HBXF peak memory usage Example Based on the HB analysis, the following example computes the transimpedance from isrc to v(1). .hb tones=1e9 nharms=4 .hbxf v(1) lin 10 1e8 1.2e8 .print hbxf tfv(isrc) tfi(n3) 290 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Transfer Function Analysis (.SNXF) HBXF Test Listing * Test HBXF: nonlinear order-2 poly equation .OPTIONS PROBE .OPTIONS POST=2 vlo lo 0 cos(0 1.0 1g 0 0) tranforhb=1 rlo lo 0 50 vrf1 rf1 0 0 rrf1 rf1 0 50 E1 out 0 POLY(2) lo 0 rf1 0 0 1 1 1 10 1 rout out 0 50 .hb tones=1g nharms=5 .hbxf v(out) lin 2 100meg 200meg .print hb v(out) v(rf1) v(lo) .print hbxf tfv(vrf1) tfv(vlo) .end Shooting Newton Transfer Function Analysis (.SNXF) The .SNXF command calculates transfer functions from an arbitrary number of small signal sources to a designated output in a circuit under periodic steady state conditions. Frequency conversion is calculated from multiple input frequencies to a single output at a single frequency that is specified on the command line. Prerequisites and Limitations The following prerequisites and limitations apply to the .SNXF command: ■ Only one .SNXF statement is required. If you use multiple .SNXF statements, HSPICE RF only uses the last one issued. ■ At least one .SN statement is required, which determines the steady-state solution. ■ Parameter sweeps must be placed in .SN statements. Input Syntax .SNXF out_var <freq_sweep> HSPICE® RF User Guide Z-2007.03 291 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Transfer Function Analysis (.SNXF) Parameter Description Parameter Description out_var Specify i(2_port_elem) or V(n1<,n2>) freq_sweep Frequency sweep range for the input signal (also referred to as the input frequency band (IFB or fin)). A sweep of type LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ LIN nsteps start stop DEC nsteps start stop ■ OCT nsteps start stop ■ POI nsteps freq_values ■ SWEEPBLOCK = BlockName Specify the frequency sweep range for the output signal. HSPICE RF determines the offset frequency in the input sidebands Fin, where Fin = abs(n*F0 +/- Fout). F0 is the steady-state fundamental tone, and Fout is the output frequency. SNXF then generates the transfer functions from all of the input sidebands (the Fin values) to the output frequency Fout. ■ Output Syntax This section describes the syntax for the SNXF .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT SNXF TYPE(NODES | ELEM) .PROBE SNXF TYPE(NODES | ELEM) Parameter Description TYPE can be one of the following: ■ TFV = existing source ■ TFI = placeholder value for the current source attached to the given node. The transfer function is computed on the output variables and input current or voltage.NODES | ELEM NODES or ELEM can be one of the following: 292 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Transfer Function Analysis (.SNXF) ■ Voltage type – a single node name (n1), or a pair of node names, (n1,n2) ■ Current type – an element name (elemname) ■ Power type – a resistor (resistorname) or port (portname) element name Output Data Files An SNXF calculation produces these output data files: ■ Output from the .PRINT statement is written to a .printsnxf# file. The output is in ohms, siemens, or undesignated units, and the header in the output file is Z(..). Y(..) or GAIN(..). ■ Output from the .PROBE statement is written to a .snxf# file. Reported performance log statistics are written to a .lis file: ■ SNXF CPU time ■ SNXF peak memory usage Example Based on the SN analysis, the following example computes the transimpedance from isrc to v(1). .SN tones=1e9 nharms=4 .SNXF v(1) lin 10 1e8 1.2e8 print SNXF TFV(isrc) TFI(n3) HSPICE® RF User Guide Z-2007.03 293 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses Shooting Newton Transfer Function Analysis (.SNXF) SNXF Test Listing * Test SNXF: nonlinear order-2 poly equation .OPTIONS PROBE .OPTIONS POST=2 vlo lo 0 cos(0 1.0 1g 0 0) rlo lo 0 50 vrf1 rf1 0 0 rrf1 rf1 0 50 E1 out 0 POLY(2) lo 0 rf1 0 0 1 1 1 10 1 rout out 0 50 .opt delmax=.01n .sn tones=1g nharms=5 .snxf v(out) lin 2 100meg 200meg .print sn v(out) v(rf1) v(lo) .print snxf tfv(vrf1) tfv(vlo) .end 294 HSPICE® RF User Guide Z-2007.03 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses References References [1] S. Maas, Nonlinear Microwave Circuits, Chapter 3, IEEE Press, 1997. [2] R. Gilmore and M.B. Steer, “Nonlinear Circuit Analysis Using the Method of Harmonic Balance - A Review of the Art, Part I, Introductory Concepts.” International Journal of Microwave and Millimeter-wave Computer-Aided Engineering, Volume 1, No. 1, pages 22-37, 1991. [3] R. Gilmore and M.B. Steer, “Nonlinear Circuit Analysis Using the Method of Harmonic Balance - A Review of the Art. Part II. Advanced Concepts.” International Journal of Microwave and Millimeter-wave Computer-Aided Engineering, Volume 1, No. 2, pages 159-180, 1991. [4] V. Rizzoli, F. Mastri, F. Sgallari, G. Spaletta, “Harmonic-Balance Simulation of Strongly Nonlinear Very Large-Size Microwave Circuits by Inexact Newton Methods,” MTT-S Digest, pages 1357-1360, 1996. [5] S. Skaggs, Efficient Harmonic Balance Modeling of Large Microwave Circuits, Ph.D. thesis, North Carolina State University, 1999. [6] R.S. Carson, High-Frequency Amplifiers, 2nd Edition, John Wiley & Sons, 1982 [7] S.Y. Liao, Microwave Circuit Analysis and Amplifier Design, Prentice-Hall, 1987. [8] Y. Saad, Iterative Methods for Sparse Linear Systems, PWS Publishing Company, 1995. [9] J. Roychowdhury, D. Long, and P. Feldmann, “Cyclostationary Noise Analysis of Large RF Circuits with Multitone Excitations,” IEEE Journal of Solid-State Circuits, volume 33, pages 324–336, March 1998. [10] A. Demir, A. Sangiovanni-Vincentelli, “Analysis and Simulation of Noise in Nonlinear Electronic Circuits and Systems”, Kluwer Academic, 1998. HSPICE® RF User Guide Z-2007.03 295 Chapter 10: Large Signal Periodic AC, Transfer Function, and Noise Analyses References 296 HSPICE® RF User Guide Z-2007.03 11 S-parameter Extraction 11 Describes how to do frequency translation and large-signal S-parameter extraction, as well as noise parameter calculation. This chapter focuses on: ■ Frequency Translation S-Parameter (HBLIN) Extraction on page 298 ■ Large-Signal S-parameter (HBLSP) Analysis on page 305 This chapter discusses various techniques supported in HSPICE RF for extracting circuit scattering parameters. Since RF circuits can operate under large-signal and small-signal conditions, there are several types of scattering parameters that are useful to measure. Linear small-signal scattering parameters represent the RF frequency-domain transfer characteristics for a circuit that is operating at its DC bias condition, but the stimulus and response signals are sufficiently small that they do not influence the operating point. This type of analysis is performed using the .LIN analysis, which is supported in both HSPICE and HSPICE RF. For information on doing small-signal S-parameter analysis (.LIN), please see Chapter 11 (Linear Network Parameter Analysis) in the HSPICE Simulation and Analysis User Guide. In the case of RF mixers and receiver front-ends, some of the input and output frequencies of interest involve a frequency translation. This translation is intentional and caused by nonlinear mixing in the circuit due to devices being driven by large-signal periodic waveforms. This type of scattering parameter analysis therefore must begin by solving the large-signal periodic response, and then finding the small-signal behavior about this large-signal operating point. This capability is provided by the .HBLIN analysis, which has setup and analysis control options similar to .LIN, but is capable of extracting S-parameters about a large-signal periodic steady-state operating point. HSPICE® RF User Guide Z-2007.03 297 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction In the case of circuits such as power amplifiers, the extraction of scattering parameters is also important, but the circuit stimulus and response signals may themselves be large-signal periodic waveforms. And, it can be important to analyze how these S-parameter vary as a function of input power levels. This capability is provided by the .HBLSP Large-Signal S-parameter analysis, which uses large-signal stimulus signals for the S-parameter extractions. Frequency Translation S-Parameter (HBLIN) Extraction Frequency translation scattering parameter (S-parameter) extraction is used to describe N-port circuits that exhibit frequency translation effects, such as mixers. The analysis is similar to the existing LIN analysis, except that the circuit is first linearized about a periodically varying operating point instead of a simple DC operating point. After the linearization, the S-parameters between circuit ports that convert signals from one frequency band to another are calculated. You use the .HBLIN statement to extract frequency translation S-parameters and noise figures. Frequency translation S-parameter describes the capability of a periodically linear time varying systems to shift signals in frequency. The S-parameters for a frequency translation system are similar to the S-parameters of a linear-timevarying system, it is defined as: Equation 62 b = S ⋅ a b i,m ( w ) S i,j;m,n ( w ) = -----------------a j,n ( w ) a k ≠ j, p ≠ n(w) =0 The incident waves, a i ,n ( w ) , and reflected waves, b i ,n ( w ) , are defined by using these equations: Equation 63 298 V i ( w + nw 0 ) + Z 0i I i ( w + nw 0 ) a i ,n ( w ) = -------------------------------------------------------------------------2 Z 0i V i ( w + nw 0 ) – Z 0i I i ( w + nw 0 ) b i ,n ( w ) = ------------------------------------------------------------------------2 Z 0i HSPICE® RF User Guide Z-2007.03 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction Where, ■ w 0 is the fundamental frequency (tone). ■ n is a signed integer. ■ i is the port number. ■ a i ,n ( w ) is the input wave at the frequency w + nw 0 on the ith port. ■ b i ,n ( w ) is the reflected wave at the frequency w + nw 0 on the ith port. ■ V i ( w + nw 0 ) is the Fourier coefficient at the frequency w + nw 0 of the voltage at port i. ■ I i ( w + wn 0 ) is the Fourier coefficient at the frequency w + nw 0 of the current at port i. ■ Z 0i is the reference impedance at port i. ■ V and I definitions are Fourier coefficients rather than phasors. For a multi-tone analysis, it can be expressed as: Equation 64 b = S⋅ a Si b i ,m ,m ...m ( w ) 1 2 N ( w ) = -------------------------------------,j;m 1 ...m N ,n 1 ,n 2 ...n N a j ,n ,n ...n ( w ) 1 HSPICE® RF User Guide Z-2007.03 2 N a k ,p ,p ...p k ≠ j ,∇ p ≠ n ( w ) 1 2 N q q = 299 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction Equation 65 N N ∑ ∑ ⎛ ⎞ ⎛ ⎞ ⎜ ⎟ ⎜ n j w j + Z 0i I i w + n j w j⎟ Vi w + ⎜ ⎟ ⎜ ⎟ ⎝ ⎠ ⎝ ⎠ j=1 j=1 a i ,n ,n ...n ( w ) = -------------------------------------------------------------------------------------------------1 2 N 2 Z oi N N ∑ ∑ ⎛ ⎞ ⎛ ⎞ ⎜ ⎟ ⎜ n j w j – Z 0i I i w + n j w j⎟ Vi w + ⎜ ⎟ ⎜ ⎟ ⎝ ⎠ ⎝ ⎠ j=1 j=1 b i ,n ,n ...n ( w ) = ----------------------------------------------------------------------------------------------1 2 N 2 Z oi Where, ■ w j is the ith tone. The frequency translate S-parameters are calculated by applying different n j ( j = 1 ∼N ) to different ports. Limitations The HBLIN analysis has these known limitations: ■ Noise parameters are not calculated for mixed-mode operation. ■ Only the S-parameters corresponding to the set of frequencies specified at each port are extracted. ■ Multiple small-signal tones are not supported. ■ The port (P) element impedance cannot be specified as complex. HB Analysis An HB analysis is required prior to an HBLIN analysis. To extract the frequency translation S-parameters, a sweep of the small-signal tone is necessary. You can identify the small-signal tone sweep in the .HBLIN command or in the .HB command together with a SS_TONE specification. For additional information regarding HB analysis, see Harmonic Balance Analysis on page 198. 300 HSPICE® RF User Guide Z-2007.03 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction Port-element You must use a port (P) element as the termination at each port of the system. To indicate the frequency band that the S-parameters are extracted from, it is necessary to specify a harmonic index for each P-element. Port Element Syntax Without SS_TONE Pxxx p n <n_ref> <PORT=portnumber > + <HBLIN = [H1, H2, ... HN, +/-1]> ... With SS_TONE Pxxx p n <n_ref> <PORT=portnumber > + <HBLIN = [H1, H2, ... +/-1 ... HN]> ... Parameter Description n_ref Reference node used when a mixed-mode port is specified. PORT The port number. Numbered sequentially beginning with 1 with no shared port numbers. HBLIN Integer vector that specifies the harmonic index corresponding to the tones defined in the .HB command. The +/-1 term corresponds to the small-signal tone specified by SS_TONE in the .HB command. If there is no SS_TONE in the .HB command, the +/-1 term must be at the last entry of HBLIN vector. HBLIN Analysis You use the .HBLIN statement to extract frequency translation S-parameters and noise figures. Input Syntax Without SS_TONE .HBLIN <frequency_sweep> + <NOISECALC = [1|0|yes|no]> <FILENAME=file_name> + <DATAFORMAT = [ri|ma|db]> + <MIXEDMODE2PORT = [dd|cc|cd|dc|sd|sc|cs|ds]> HSPICE® RF User Guide Z-2007.03 301 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction With SS_TONE .HBLIN <NOISECALC = [1|0|yes|no]> <FILENAME=file_name> + <DATAFORMAT = [ri|ma|db]> + <MIXEDMODE2PORT = [dd|cc|cd|dc|sd|sc|cs|ds]> Parameter Description frequency_sweep Frequency sweep range for the input signal (also referred to as the input frequency band (IFB) or fin). You can specify LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ ■ ■ ■ ■ ■ NOISECALC Enables calculating the noise figure. The default is no (0). FILENAME Specifies the output file name for the extracted S-parameters or the object name after the -o command-line option. The default is the netlist file name. DATAFORMAT Specifies the format of the output data file. ■ ■ ■ 302 LIN nsteps start stop DEC nsteps start stop OCT nsteps start stop POI nsteps freq_values SWEEPBLOCK nsteps freq1 freq2 ... freqn DATA=dataname dataformat=RI, real-imaginary. dataformat=MA, magnitude-phase. This is the default format for Touchstone files. dataformat=DB, DB(magnitude)-phase. HSPICE® RF User Guide Z-2007.03 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction Parameter Description MIXEDMODE2PORT Describes the mixed-mode data map of output mixed mode Sparameter matrix. The availability and default value for this keyword depends on the first two port (P element) configuration as follows: ■ ■ ■ ■ case 1: p1=p2=single-ended (standard-mode P element) available: ss default: ss case 2: p1=p2=balanced (mixed-mode P element) available: dd, cd, dc, cc default: dd case 3: p1=balanced p2=single-ended available: ds, cs default: ds case 4: p1=single p2=balanced available: sd, sc default: sd Example 1 Single-tone analysis with frequency translation. In this example, the 2-port Sparameters from RF (1G-del_f) to IF (del_f) are extracted. The LO signal is specified by normal voltage source Vlo. The frequency on port 1 is in the RF band, 1G-del_f, and the frequency on port 2 is in the IF band, del_f. The IF band is swept from 0- to 100-MHz. The results are output to file ex1.s2p. p1 RFin gnd port=1 HBLIN=(1,-1) p2 IFout gnd port=2 HBLIN=(0,1) Vlo LOin gnd DC 0 HB 2.5 0 1 1 .HB tones=1G harms=5 .HBLIN lin 5 0 100meg noisecalc=no filename=ex1 + dataformat=ma Example 2 Another single-tone analysis with frequency translation example. In this example, the 3-port S-parameters are extracted. Port 3 provides the periodic large signal. The frequency on port 1 is del_f, the frequency on port 2 is 1G*2-del_f, and the frequency on port 3 is 1G*1+del_f. The small-signal frequency is swept from 0 to 100MHz. HBNOISE calculation is required. The results are output to file ex2.s3p. HSPICE® RF User Guide Z-2007.03 303 Chapter 11: S-parameter Extraction Frequency Translation S-Parameter (HBLIN) Extraction p1 1 0 port=1 HBLIN=(0, 1) p2 2 0 port=2 HBLIN=(2, -1) p3 3 0 port=3 hb 0.5 0 1 1 HBLIN=(1, 1) .HB tones=1G harms=5 .HBLIN lin 5 0 100meg noisecalc=yes filename=ex2 Output Syntax This section describes the syntax for the HBLIN .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT .PROBE .PRINT .PROBE .PRINT .PROBE HBLIN Smn | Smn(TYPE) | S(m,n) | S(m,n)(TYPE) HBLIN Smn | Smn(TYPE) | S(m, n) | S(m, n)(TYPE) HBLIN SXYmn | SXYmn(TYPE) | SXY(m,n) | SXY(m,n)(TYPE) HBLIN SXYmn | SXYmn(TYPE) | SXY(m, n) | SXY(m, n)(TYPE) HBLIN <NF> <SSNF> <DSNF> HBLIN <NF> <SSNF> <DSNF> Parameter Description Smn | Smn(TYPE) | Complex 2-port parameters. Where: S(m,n) | S(m,n)(TYPE) ■ m = 1 or 2 SXYmn | SXYmn(TYPE) | ■ n = 1 or 2 SXY(m,n) | SXY(m,n)(TYPE) ■ X and Y are used for mixed-mode S-parameter output. The values for X and Y can be D (differential), C (common), or S (single-end). ■ TYPE = R, I, M, P, PD, D, DB, or DBM R = real I = imaginary M = magnitude P = PD = phase in degrees D = DB = decibels DBM = decibels per 1.0e-3 304 HSPICE® RF User Guide Z-2007.03 Chapter 11: S-parameter Extraction Large-Signal S-parameter (HBLSP) Analysis Parameter Description NF SSNF NF and SSNF both output a single-side band noise figure as a function of the IFB points: NF = SSNF = 10 Log(SSF) Single side-band noise factor, SSF = {(Total Noise at output, at OFB, originating from all frequencies) - (Load Noise originating from OFB)} / (Input Source Noise originating from IFB). DSNF DSNF outputs a double side-band noise figure as a function of the IFB points. DSNF = 10 Log(DSF) Double side-band noise factor, DSF = {(Total Noise at output, at the OFB, originating from all frequencies) (Load Noise originating from the OFB)} / (Input Source Noise originating from the IFB and from the image of IFB). Output Data Files An HBLIN analysis produces these output data files: ■ The S-parameters from the .PRINT statement are written to a .printhl# file. ■ The extracted S-parameters from the .PROBE statement are written to a .hl# file. Large-Signal S-parameter (HBLSP) Analysis An HBLSP analysis provides three kinds of analyses for periodically-driven nonlinear circuits, such as those that employ power amplifiers and filters: ■ Two-port power-dependant (large-signal) S-parameter extraction ■ Two-port small-signal S-parameter extraction ■ Two-port small-signal noise parameter calculation Unlike small-signal S-parameters, which are based on linear analysis, powerdependent S-parameters are based on harmonic balance simulation. Its solution accounts for nonlinear effects such as compression and variation in power levels. HSPICE® RF User Guide Z-2007.03 305 Chapter 11: S-parameter Extraction Large-Signal S-parameter (HBLSP) Analysis The definition for power-dependent S-parameters is similar to that for smallsignal parameters. Power-dependent S-parameters are defined as the ratio of reflected and incident waves by using this equation: b=S*a ; S[i, j]=b[i,n]/a[j,n] when a[k,n](k!=j)=0 The incident waves, a[i, n], and reflected waves, b[i, n], are defined by using these equations: a[i, n] = (V[i](n*W0) + Zo[i] * I[i](n*W0)) / (2 * sqrt(Zo[i])) b[i, n] = (V[i](n*W0) - Zo[i] * I[i](n*W0)) / (2 * sqrt(Zo[i])) Where: ■ W0 is the fundamental frequency (tone). ■ n is a signed integer. ■ i is the port number. ■ a[i, n] is the input wave at the frequency n*W0 on the ith port. ■ b[i, n] is the reflected wave at the frequency n*W0 on the ith port. ■ V[i](n*W0) is the Fourier coefficient at the frequency n*W0 of the voltage at port i. ■ I[i](n*W0) is the Fourier coefficient at the frequency n*W0 of the current at port i. ■ Zo[i] is the reference impedance at port i. An HBLSP analysis only extracts the S-parameters on the first harmonic (that is, n=1). Limitations The HBLSP analysis has these known limitations: 306 ■ Power-dependent S-parameter extraction is a 2-port analysis only. Multiport power-dependent S-parameters are not currently supported. ■ The intermodulation data block (IMTDATA) in the .p2d# file is not supported. ■ The internal impedance of the P (port) Element can only be a real value. Complex impedance values are not supported. HSPICE® RF User Guide Z-2007.03 Chapter 11: S-parameter Extraction Large-Signal S-parameter (HBLSP) Analysis Input Syntax .HBLSP NHARMS=nh <POWERUNIT=[dbm | watt]> + <SSPCALC=[1|0|YES|NO]> <NOISECALC=[1|0|YES|NO]> + <FILENAME=file_name> <DATAFORMAT=[ri | ma | db]> + FREQSWEEP freq_sweep POWERSWEEP power_sweep Parameter Description NHARMS Number of harmonics in the HB analysis triggered by the .HBLSP statement. POWERUNIT Power unit. Default is watt. SSPCALC Extract small-signal S-parameters. Default is 0 (NO). NOISECALC Perform small-signal 2-port noise analysis. Default is 0 (NO). FILENAME Output data .p2d# filename. Default is the netlist name or the object name after the -o command-line option. DATAFORMAT Format of the output data file. Default is ma (magnitude, angle). FREQSWEEP Frequency sweep specification. A sweep of type LIN, DEC, OCT, POI, or SWEEPBLOCK. Specify the nsteps, start, and stop times using the following syntax for each type of sweep: ■ LIN nsteps start stop DEC nsteps start stop ■ OCT nsteps start stop ■ POI nsteps freq_values ■ SWEEPBLOCK=blockname This keyword must appear before the POWERSWEEP keyword. ■ POWERSWEEP Power sweep specification. A sweep of type LIN, DEC, OCT,POI, or SWEEPBLOCK. Specify the nsteps, start, and stop frequencies using the following syntax for each type of sweep: ■ LIN nsteps start stop DEC nsteps start stop ■ OCT nsteps start stop ■ POI nsteps power_values ■ SWEEPBLOCK=blockname This keyword must follow the FREQSWEEP keyword. ■ HSPICE® RF User Guide Z-2007.03 307 Chapter 11: S-parameter Extraction Large-Signal S-parameter (HBLSP) Analysis Note: The FREQSWEEP and POWERSWEEP keywords must appear at the end of an .HBLSP statement. Examples Example 1does 2-port single-tone, power-dependent S-parameter extraction, without frequency translation: ■ Frequency sweep: The fundamental tone is swept from 0 to 1G ■ Power sweep: The power input at port 1 is swept from 6 to 10 Watts. ■ Five harmonics are required for the HB analysis. Large-signal S-parameters are extracted on the first harmonic. ■ Five harmonics are required in the HBLSP triggered HB analysis. ■ The DC value in p1 statement is used to set DC bias, which is used to perform small-signal analyses. ■ Small-signal S-parameters are required extracted. ■ Small-signal two-port noise analysis is required. ■ The data will be output to the ex1.p2d file. Example 1 2-Port, Single Tone p1 1 0 port=1 dc=1v p2 2 0 port=2 .hblsp nharms=5 powerunit = watt + sspcalc=1 noisecalc=1 filename=ex1 + freqsweep lin 5 0 1G powersweep lin 5 6 10 Example 2 generates large scale S-parameters as a function of input for a differential equalizer. Example 2 4-Port Network * hblsp example .opt post p1 n1 0 port=1 ac=1 p2 n2 0 port=2 *** put your DUT R1 n1 n2 10*** .hblsp nharms=5 + freqsweep lin 4 1k 10k + powersweep lin 2 5 10 .end 308 HSPICE® RF User Guide Z-2007.03 Chapter 11: S-parameter Extraction Large-Signal S-parameter (HBLSP) Analysis Output Syntax This section describes the syntax for the HBLSP .PRINT and .PROBE statements. These statements only support S and noise parameter outputs. Node voltage, branch current, and all other parameters are not supported in HBLSP .PRINT and .PROBE statements. .PRINT and .PROBE Statements .PRINT HBLSP Smn | Smn(TYPE) | + ...small signal 2-port noise .PROBE HBLSP Smn | Smn(TYPE) | + ...small signal 2-port noise S(m, n) | S(m, n)(TYPE) params... S(m, n) | S(m, n)(TYPE) params... Parameter Description Smn | Smn(TYPE) | S(m,n) | S(m,n)(TYPE) Complex 2-port parameters. Where: ■ ■ ■ ... small signal 2-port noise parameters ... m = 1 or 2 n = 1 or 2 TYPE = R, I, M, P, PD, D, DB, or DBM R = real I = imaginary M = magnitude P = PD = phase in degrees D = DB = decibels DBM = decibels per 1.0e-3 G_AS | NF | RN | YOPT | GAMMA_OPT | NFMIN | VN2 | ZCOR | GN | RHON | YCOR | ZOPT | IN2 For a description of these parameters, see Linear Network Parameter Analysis in the HSPICE Simulation and Analysis User Guide. Output Data Files An HBLSP analysis produces these output data files: ■ The large-signal S-parameters from the .PRINT statement are written to a .printls# file. ■ The small-signal S-parameters from the .PRINT statement are written to a .printss# file. HSPICE® RF User Guide Z-2007.03 309 Chapter 11: S-parameter Extraction Large-Signal S-parameter (HBLSP) Analysis ■ The large-signal S-parameters from the .PROBE statement are written to a .ls# file. ■ The small-signal S-parameters from the .PROBE statement are written to a .ss# file. ■ The extracted large- and small-signal S and noise parameters are written to a .p2d# file. The large- and small-signal S-parameters from the .PROBE statement are viewable in CosmosScope. 310 HSPICE® RF User Guide Z-2007.03 12 12 Envelope Analysis Describes how to use envelope simulation. Envelope Simulation Envelope simulation combines features of time- and frequency-domain analysis. Harmonic Balance (HB) solves for a static set of phasors for all the circuit state variables, as shown in this equation: N Equation 66 v ( t ) = a0 + ∑ [ ai cos ωi t + bi sin ωi t ] i=1 In contrast, envelope analysis finds a dynamic, time-dependent set of phasors, as this equation shows: Equation 67 v ( t ) = a 0 ( ˆt ) + N ∑ [ ai (ˆt ) cos ωi t + bi (ˆt ) sin ωi t ] i=1 Thus, in envelope simulation, each signal is described by the evolving spectrum. Envelope analysis is generally used on circuits excited by signals with significantly different timescales. An HB simulation is performed at each point in time of the slower-moving ( ˆt ) timescale. In this way, for example, a 2tone HB simulation can be converted into a series of related 1-tone simulations where the transient analysis proceeds on the ( ˆt ) timescale, and 1-tone HB simulations are performed with the higher frequency tone as the fundamental frequency. In HSPICE RF, any voltage or current source identified as a HB source either in a V or I element statement, or by an .OPTION TRANFORHB command, is used HSPICE® RF User Guide Z-2007.03 311 Chapter 12: Envelope Analysis Envelope Simulation for HB simulations at each point in ˆt time. All other sources are associated with the transient timescale. Also, the input waveforms can be represented in the frequency domain as RF carriers modulated by an envelope by identifying a VMRF signal source in a V or I element statement. The amplitude and phase values of the sampled envelope are used as the input signal for HB analysis. Some typical applications for envelope simulation are amplifier spectral regrowth, adjacent channel power ration (ACPR), and oscillator startup and shutdown analyses. Envelope Analysis Commands This section describes those commands specific to envelope analysis. These commands are: ■ Standard envelope simulation (.ENV) ■ Oscillator simulation, both startup and shutdown (.ENVOSC) ■ Envelope Fast Fourier Transform (.ENVFFT) Nonautonomous Form .ENV TONES=f1<f2...fn> NHARMS=h1<h2...hn> + ENV_STEP=tstep ENV_STOP=tstop Parameter Description TONES Carrier frequencies, in hertz. NHARMS Number of harmonics. ENV_STEP Envelope step size, in seconds. ENV_STOP Envelope stop time, in seconds. Description You use the .ENV command to do standard envelope simulation. The simulation proceeds just as it does in standard transient simulation, starting at time=0 and continuing until time=env_stop. An HB analysis is performed at each step in time. You can use Backward-Euler (BE), trapezoidal (TRAP), or level-2 Gear (GEAR) integration. Recommended option settings are: 312 HSPICE® RF User Guide Z-2007.03 Chapter 12: Envelope Analysis Envelope Simulation ■ For BE integration, set .OPTION SIM_ORDER=1. ■ For TRAP, set .OPTION SIM_ORDER=2 (default) METHOD=TRAP (default). ■ For GEAR, set .OPTION SIM_ORDER=2 (default) METHOD=GEAR. Example .env tones=1e9 nharms=6 env_step=10n env_stop=1u Oscillator Analysis Form .ENVOSC TONE=f1 NHARMS=h1 ENV_STEP=tstep ENV_STOP=tstop + PROBENODE=n1,n2,vosc <FSPTS=num, min, max> Parameter Description TONE Carrier frequencies, in hertz. NHARMS Number of harmonics. ENV_STEP Envelope step size, in seconds. ENV_STOP Envelope stop time, in seconds. PROBENODE Defines the nodes used for oscillator conditions and the initial probe voltage value. FSPTS Specifies the frequency search points used in the initial smallsignal frequency search. Usage depends on oscillator type. Description You use the .ENVOSC command to do envelope simulation for oscillator startup or shutdown. Oscillator startup or shutdown analysis with this command must be helped along by converting a bias source from a DC description to a PWL description that either: ■ Starts at a low value that supports oscillation and ramps up to a final value (startup simulation) ■ Starts at the DC value and ramps down to zero (shutdown simulation). In addition to solving for the state variables at each envelope time point, the .ENVOSC command also solves for the frequency. This command is intended to be applied to high-Q oscillators that take a long time to reach steady-state. For these circuits, standard transient analysis is too costly. Low-Q oscillators, such HSPICE® RF User Guide Z-2007.03 313 Chapter 12: Envelope Analysis Envelope Simulation as typical ring oscillators, are more efficiently simulated with standard transient analysis. Example .envosc tone=250Meg nharms=10 env_step=20n env_stop=10u + probenode=v5,0,1.25 Fast Fourier Transform Form .ENVFFT <output_var> <NP=value> <FORMAT=keyword> + <WINDOW=keyword> <ALFA=value> Parameter Description output_var Any valid output variable. NP The number of points to use in the FFT analysis. NP must be a power of 2. If not a power of 2, then it is automatically adjusted to the closest higher number that is a power of 2. The default is 1024. FORMAT Specifies the output format: NORM= normalized magnitude UNORM=unnormalized magnitude (default) WINDOW Specifies the window type to use: RECT=simple rectangular truncation window (default) BART=Bartlett (triangular) window HANN=Hanning window HAMM=Hamming window BLACK=Blackman window HARRIS=Blackman-Harris window GAUSS=Gaussian window KAISER=Kaiser-Bessel window ALFA Controls the highest side-lobe level and bandwidth for GAUSS and KAISER windows. The default is 3.0. Description You use the .ENVFFT command to perform Fast fourier Transform (FFT) on envelope output. This command is similar to the .FFT command. The only difference is that transformation is performed on real data with the .FFT command, and with the .ENVFFT command, the data being transformed is 314 HSPICE® RF User Guide Z-2007.03 Chapter 12: Envelope Analysis Envelope Simulation complex. You usually want to do this for a specific harmonic of a voltage, current, or power signal. Example .envfft v(out)[1] Output Syntax The results from envelope simulation can be made available through the .PRINT, .PROBE, and .MEASURE commands. This section describes the basic syntax you can use for this purpose. .PRINT or .PROBE You can print or probe envelope simulation results by using the following commands: .PRINT ENV ov1 <ov2... > .PROBE ENV ov1 <ov2... > Where ov1... are the output variables to print or probe. .MEASURE In HSPICE RF, the independent variable for envelope simulation is the first tone. Otherwise and except for the analysis type, the .MEASURE statement syntax is the same as the syntax for HB; for example, .MEASURE ENV result ... Envelope Output Data File Format The results of envelope simulations are written to *.ev# data files by the .PROBE statement. The format of an *.ev# data file is equivalent to an *.hb# data file with the addition of one fundamental parameter sweep that represents the slowly-varying time-envelope variation ˆt of the Fourier coefficients and frequencies. You can recognize this swept parameter” in the *.ev# file by the keyword env_time. Each row in the tabulated data of an *.ev# file includes values for identifying frequency information, the complex data for the output variables, and information on the envelope time sweep. For example, the header for a data file HSPICE® RF User Guide Z-2007.03 315 Chapter 12: Envelope Analysis Envelope Simulation dump for output variables v(in) and v(out) that follow a 2-tone envelope analysis, have entries for: hertz v(in) v(out) n0 f0 n1 f1 sweep env_time $&%# Which result in data blocks with floating point values following: env_time[0] f[0] a[0]{v(in)} b[0] {v(in)} a[0] {v(out)} b[0] {v(out)} n0 f0 n1 f1 f[1] a[1]{v(in)} b[1] {v(in)} a[1] {v(out)} b[1] {v(out)} n0 f0 n1 f1 ... f[N] a[N]{v(in)} b[N] {v(in)} a[N] {v(out)} b[N] {v(out)} n0 f0 n1 f1 env_time[1] f[0] a[0]{v(in)} b[0] {v(in)} a[0] {v(out)} b[0] {v(out)} n0 f0 n1 f1 f[1] a[1]{v(in)} b[1] {v(in)} a[1] {v(out)} b[1] {v(out)} n0 f0 n1 f1 ... f[N] a[N]{v(in)} b[N] {v(in)} a[N] {v(out)} b[N] {v(out)} n0 f0 n1 f1 ... env_time[M-1] f[0] a[0]{v(in)} b[0] {v(in)} a[0] {v(out)} b[0] {v(out)} n0 f0 n1 f1 f[1] a[1]{v(in)} b[1] {v(in)} a[1] {v(out)} b[1] {v(out)} n0 f0 n1 f1 ... f[N] a[N]{v(in)} b[N] {v(in)} a[N] {v(out)} b[N] {v(out)} n0 f0 n1 f1 Where there are M data blocks corresponding to M envelope time points, with each block containing N+1 rows for the frequency data. The units for the env_time sweep are seconds. 316 HSPICE® RF User Guide Z-2007.03 13 Post-Layout Analysis 13 Describes the post-layout analysis flow, including post-layout back-annotation, DSPF and SPEF files, linear acceleration, check statements, and power analysis. Post-Layout Back-Annotation A traditional, straightforward, “brute-force” flow runs an RC extraction tool that produces a detailed standard parasitic format (DSPF) file. DSPF is the standard format for transferring RC parasitic information. This traditional flow then feeds this DSPF file into the circuit simulation tool for post-layout simulation. A key problem is that the DSPF file is flat. Accurately simulating a complete design, such as an SRAM or an on-chip cache, is a waste of workstation memory, disc space usage, and simulation runtime. Because this DSPF file is flat, control and analysis are limited. ■ How do you set different options for different blocks for better trade-off between speed and accuracy? ■ How do you perform a power analysis on a flat netlist to check the power consumption? ■ This traditional flow flattens all nodes after extraction so it is more difficult to compare the delay before and after extraction. ■ This traditional flow can also stress the limits of an extraction tool so reliability also becomes an issue. HSPICE RF provides a flow that solves all of these problems. HSPICE® RF User Guide Z-2007.03 317 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation ■ Star-RCXT generates a hierarchical Layout Versus Schematic (LVS) ideal netlist, and flat information about RC parasitics in a DSPF or (standard parasitic exchange format (SPEF) file. ■ HSPICE RF uses the hybrid flat-hierarchical approach to back-annotate the RC parasitics, from the DSPF or SPEF file, into the hierarchical LVS ideal netlist. Using the hierarchical LVS ideal netlist cuts simulation runtime and CPU memory usage. Because HSPICE RF uses the hierarchical LVS ideal netlist as the top-level netlist, you can fully control the netlist. For example: ■ You can set different modes to different blocks for better accuracy and speed trade-off. ■ You can run power analysis, based on the hierarchical LVS ideal netlist, to determine the power consumption of each block. If you use the hierarchical LVS ideal netlist, you can reuse all post-processing statements from the prelayout simulation for the post-layout simulation. This saves time, and the capacity of the verification tool is not stressed so reliability is higher. HSPICE RF supports only the XREF:COMPLETE flow and the XREF:NO flow from Star-RCXT. Refer to the Star-RCXT User Guide for more information about the XREF flow. To generate a hierarchical LVS ideal netlist with Star-RCXT, include the following options in the Star-RCXT command file. *** for XREF:NO flow *** NETLIST_IDEAL_SPICE_FILE: ideal_spice_netlist.sp NETLIST_IDEAL_SPICE_TYPE: layout NETLIST_IDEAL_SPICE_HIER:YES *** for XREF:COMPLETE flow *** NETLIST_IDEAL_SPICE_FILE: ideal_spice_netlist.sp NETLIST_IDEAL_SPICE_TYPE: schematic NETLIST_IDEAL_SPICE_HIER:YES Note: Before version 2002.2, Star-RCXT used NETLIST_IDEAL_SPICE_SKIP_CELLS to generate the hierarchical ideal SPICE netlist. HSPICE RF can still simulate post-layout designs using the brute-force flow, but the post-layout flow is preferable in HSPICE RF. 318 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation HSPICE RF supports these post-layout flows to address your post-layout simulation needs. ■ Standard Post-Layout Flow ■ Selective Post-Layout Flow ■ Additional Post-Layout Options Standard Post-Layout Flow Use this flow mainly for analog or mixed signal design, and high-coverage verification runs when you need to back-annotate RC parasitics into the hierarchical LVS ideal netlist. In this flow, HSPICE RF expands all nets from the DSPF or SPEF file. To expand only selected nets, use see Selective PostLayout Flow on page 322. Figure 23 Standard Post-Layout Flow Extraction Tool Ideal Netlist DSPF SPEF HSPICE RF Back-annotation .html .lis HSPICE® RF User Guide Z-2007.03 319 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Standard Post-Layout Flow Control Options The standard post-layout flow options are SIM_DSPF and SIM_SPEF. Include one of these options in your netlist. For example, .OPTION SIM_DSPF=“[scope] dspf_filename” .OPTION SIM_SPEF=“spec_filename” In the SIM_DSPF syntax, scope can be a subcircuit definition or an instance. If you do not specify scope, it defaults to the top-level definition. HSPICE RF requires both a DSPF file and an ideal netlist. Only flat DSPF files are supported; hierarchy statements, such as .SUBCKT and .x1, are ignored. Very large circuits generate very large DSPF files; this is when using either the SIM_DSPF or the SIM_DSPF_ACTIVE option can really improve performance. You can specify a DSPF file in the SIM_SPEF option, or a SPEF file in the SIM_DSPF option. The scope function is not supported in the SPEF format. For descriptions and usage examples, see .OPTION SIM_DSPF and .OPTION SIM_SPEF in the HSPICE and HSPICE RF Command Reference. 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 SIM_DSPF With SIM_LA Option The SIM_DSPF option accelerates the simulation by more than 100%. By using the SIM_LA option at the same time, you can further reduce the total CPU time: $ 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 320 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation 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. For syntax and description of SIM_DSPF_ACTIVE option, see .OPTION SIM_DSPF_ACTIVE in the HSPICE and RF Command Reference. 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 HSPICE® RF User Guide Z-2007.03 321 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Selective Post-Layout Flow Figure 24 Selective Post-Layout Flow Extraction Tool DSPF SPEF Ideal Netlist HSPICE RF Active Nodes Back-annotation HSPICE RF .html .lis You can use the selective post-layout flow to simulate a post-layout design for a memory or digital circuit, and for a corner-point verification run. Instead of backannotating all RC parasitics into the ideal netlist, the selective post-layout flow automatically detects and back-annotates only active parasitics, into the hierarchical LVS ideal netlist. For a high-latency design, the selective postlayout flow is an order of magnitude faster than the standard post-layout flow. 322 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Note: The selective post-layout flow applies only to RF transient analyses and cannot be used with other analyses such as DC, AC, or HB. Selective Post-Layout Flow Control Options To invoke the selective post-layout flow, include one of the options listed in Table 23 in your netlist. Table 23 Selective Post-Layout Flow Options Syntax Description SIM_DSPF_ACTIVE -orSIM_SPEF_ACTIVE HSPICE RF performs a preliminary verification run to determine the activity of the nodes and generates two ASCII files: active_node.rc and active_node.rcxt. These files save all active node information in both Star-RC format and StarRCXT format. By default, a node is considered active if the voltage varies by more than 0.1V. To change this value, use the SIM_DSPF_VTOL or SIM_SPEF_VTOL option. For descriptions and usage examples, see .OPTION SIM_DSPF_ACTIVE and .OPTION SIM_SPEF_ACTIVE in the HSPICE and RF Command Reference. SIM_DSPF_VTOL -orSIM_SPEF_VTOL HSPICE RF performs a second simulation run by using the active_node file, the DSPF or SPEF file, and the hierarchical LVS ideal netlist to back-annotate only active portions of the circuit. If a net is latent, then HSPICE RF does not expand the net. This saves simulation runtime and memory. ■ value is the tolerance of the voltage change. scopen can be a subcircuit definition (which has an @ prefix), or a subcircuit instance. By default, HSPICE RF performs only one iteration of the second simulation run. Use the SIM_DSPF_MAX_ITER or SIM_SPEF_MAX_ITER option to change it. ■ For descriptions and usage examples, see .OPTION SIM_DSPF_VTOL and .OPTION SIM_SPEF_VTOL in the HSPICE and HSPICE RF Command Reference. HSPICE® RF User Guide Z-2007.03 323 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 23 Selective Post-Layout Flow Options (Continued) Syntax Description SIM_DSPF_MAX_ITER value is the maximum number of iterations for the second -orsimulation run. SIM_SPEF_MAX_ITER Some of the latent nets might turn active after the first iteration of the second run. In this case: ■ Resimulate the netlist to ensure the accuracy of the postlayout simulation. ■ Use SIM_DSPF_MAX_ITER or SIM_SPEF_MAX_ITER to set the maximum number of iterations for the second run. If the active_node remains the same after the second simulation run, HSPICE RF ignores these options. For descriptions and usage examples, see .OPTION SIM_DSPF_MAX_ITER and .OPTION SIM_SPEF_MAX_ITER in the HSPICE and HSPICE RF Command Reference. Additional Post-Layout Options Other post-layout options are listed in Table 24. Table 24 Additional Post-Layout Options Syntax Description SIM_DSPF_RAIL -orSIM_SPEF_RAIL By default, HSPICE RF does not back-annotate parasitics of the power-net. To back-annotate power-net parasitics, include one of these options in the netlist. Default=OFF. ON expands nets in a power rail as it expands all nets. SIM_DSPF_SCALER SIM_SPEF_SCALER -orSIM_DSPF_SCALEC SIM_SPEF_SCALEC 324 Scales the resistance or capacitance values. ■ ■ scaleR is the scale factor for resistance scaleC is the scale factor for capacitance. HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 24 Additional Post-Layout Options (Continued) Syntax Description SIM_DSPF_LUMPCAPS If HSPICE RF cannot back-annotate an instance in a net -orbecause one or more instances are missing in the SIM_SPEF_LUMPCAPS hierarchical LVS ideal netlist, then by default HSPICE RF does not evaluate the net. Instead of ignoring all parasitic information for this net, HSPICE RF includes these options to connect a lumped capacitor with a value equal to the net capacitance to this net. Default = ON adds lumped capacitance; ignores other net contents. SIM_DSPF_INSERROR HSPICE RF supports options to skip the unmatched -orinstance, and continue the evaluation of the next instance. SIM_SPEF_INSERROR The default is OFF. ON skips unmatched instances and continues the evaluation. SIM_SPEF_PARVALUE This option affects only values in a SPEF file that have triplet format: float:float:float, which this option interprets as best:average:worst. In such cases: ■ ■ ■ If SIM_SPEF_PARVALUE=1, HSPICE RF uses best. If SIM_SPEF_PARVALUE=2 (default), HSPICE RF uses average. If SIM_SPEF_PARVALUE=3, HSPICE RF uses worst. Unsupported SPEF Options HSPICE RF does not yet support the following IEEE-481 SPEF options: ■ Hierarchical SPEF definition (multiple SPEF files connected with a hierarchical definition): ■ *DEFINE and *PDEFINE ■ *R_NET and *R_PNET definition ■ *D_PNET definition. HSPICE® RF User Guide Z-2007.03 325 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Selective Extraction Flow Use the selective extraction flow if disk space is limited. Especially use this option when simulating a full-chip post-layout design, where block latency is high. HSPICE RF feedbacks the active net information to Star-RCXT to extract only the active parasitic. The major advantage of this flow is a smaller DSPF or SPEF file, which saves disk space. Figure 25 Selective Extraction Flow Star-RCXT DSPF/SPEF Post-Layout Flow Ideal Netlist OR HSPICE RF Active Nodes Star-RCXT DSPF/SPEF Post-Layout Flow Note: HSPICE RF generates an active node file in both Star-RC and Star-RCXT format. It then expands the active node file to the Star-RCXT command file to extract only active parasitics. 326 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Overview of DSPF Files In general, an SPF (Standard Parasitic Format) file describes interconnect delay and loading, due to parasitic resistance and capacitance. DSPF (Detailed Standard Parasitic Format) is a specific type of SPF file that describes the actual parasitic resistance and capacitance components of a net. DSPF is a standard output format commonly used in many parasitic extraction tools, including Star-RCXT. The HSPICE RF circuit simulator can read DSPF files. DSPF File Structure The DSPF standard is published by Open Verilog International (OVI). For information about how to obtain the complete DSPF specification, or any other documents from OVI, see: http://www.ovi.org/document.html The OVI DSPF specification requires the following file structure in a DSPF file. Parameters in {braces} are optional: HSPICE® RF User Guide Z-2007.03 327 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation DSPF_file : := *|DSPF{version} {*|DESIGN design_name} {*|DATE date} {*|VENDOR vendor} {*|PROGRAM program_name} {*|VERSION program_version} {*|DIVIDER divider} {*|DELIMITER delimiter} .SUBCKT *|GROUND_NET {path divider} net_name *|NET {path divider} net_name || {path divider} instance_name || pin_name net_capacitance *|P (pin_name pin_type pinCap {resistance {unit} {O} capacitance {unit} {F}} {x_coordinate y_coordinate}) || *|I {path divider} instance_name delimiter pin_name {path divider} instance_name pin_name pin_type pinCap {resistance {unit} {O} capacitance {unit}{F}} {x_coordinate y_coordinate} *|S ({path divider} net_name || {path divider} instance_name delimiter pin_name || pin_name instance_number {x_coordinate y_coordinate}) capacitor_statements resistor_statements subcircuit_call_statements .ENDS 328 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation {.END} Table 25 DSPF Parameters Parameter Definition *|DSPF Specifies that the file is in DSPF format. {version} Version number of the DSPF specification (optional). *| Words that start with *| are keywords. || Or (use the option either preceding or following ||). For example, *|P || *I means you can use either the *|P option or the *|I option. design_name Name of your circuit design (optional). date Date and time when a parasitic extraction tool (such as StarRCXT) generated the DSPF file (optional). vendor Name of the vendor (such as Synopsys) whose tools you used to generate the DSPF file (optional). program_name Name of the program (such as Star-RCXT) that generated the DSPF file (optional). program_version Version number of the program that generated the DSPF file (optional). divider Character that divides levels of hierarchy in a circuit path (optional). If you do not define this parameter, the default hierarchy divider is a slash (/). For example, X1/X2 indicates that X2 is a subcircuit of the X1 circuit. delimiter Character used to separate the name of an instance and a pin in a concatenated instance pin name, or a net name and a sub-node number in a concatenated sub-node name. If you do not define this parameter, the default delimiter is a colon (:). path Hierarchical path to a net, instance, or pin, within a circuit. net_name Name of a net in a circuit or subcircuit. HSPICE® RF User Guide Z-2007.03 329 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 25 DSPF Parameters (Continued) Parameter Definition instance_name Name of an instance of a subcircuit. pin_name Name of a pin on an instance of a subcircuit. pinCap Capacitance of a pin. pin_type ■ ■ ■ ■ ■ ■ resistance I (input) O (output) B (bidirectional) X (don’t care) S (switch) J (jumper) Resistance on a pin in ohms for input (I), output (O), or bidirectional (B) pins. You can use resistance-capacitance (RC) pairs to model pin characteristics by using a higherorder equivalent RC ladder circuit than a single capacitor model. For example: C0 {R1 C1 R2 C2...}. Attaching RC pairs increases the order of the equivalent circuit from the first (C0) order. For X, S, and J pin types, simulation ignores this generalized capacitance value, but you should insert a 0 value as a place-holder for format integrity. The resistance value can be a real number or an exponent (optionally followed by a real number). You can enter an O (ohms) after the value. capacitance Capacitance on a pin in farads for input (I), output (O), or bidirectional (B) pins. Use as part of a resistancecapacitance (RC) pair. Optionally enter an F (farads) after the value. unit ■ ■ ■ ■ ■ ■ 330 K (kilo) M (milli) U (micro) N (nano) P (pico) F (femto) x_coordinate Location of a pin relative to the x (horizontal) axis. y_coordinate Location of a pin relative to the y (vertical) axis. HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 25 DSPF Parameters (Continued) Parameter Definition capacitor_ statements SPICE-type statements that define capacitors in the subcircuit. resistor_ statements SPICE-type statements that define resistors in the subcircuit. subcircuit_call_ statements Statements that call the subcircuit from higher-level circuits. .END Marks the end of the file (optional). HSPICE® RF User Guide Z-2007.03 331 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation DSPF File Example *|DSPF 1.0 *|DESIGN "my_circuit" *|DATE June 15, 2002 14:12:43 *|VENDOR "Synopsys" *|PROGRAM "Star-RC" *|VERSION "Star-RCXT 2002.2" *|DIVIDER / *|DELIMITER : .SUBCKT BUFFER OUT IN * Description of Nets *GROUND_NET VSS *|NET IN 1.221451PF *|P(IN 1 0.0 0 10) *|I(DF1:A DF1 A I 0.0PF 10.0 10.0) *|I(DF1:B DF1 B I 0.0PF 10 0 20.0) *|S(IN:1 5.0 10.0)(IN:2 5.0 20.0) C1 IN VSS 0.117763PF C2 IN:1 VSS 0.276325PF C3 IN:2 VSS 0.286325PF C4 DF1:A VSS 0.270519PF C5 DF1:B VSS 0.270519PF R20 IN N:1 1.70333E00 R21 IN:1 DF1:A 1.29167E-01 R22 IN:1 IN:2 1.29167E-01 R23 IN:2 DF1:B 1.70333E-01 *|NET BF 0.287069PF *|I(DF1:C DF1 C O 0.0PF 12.0 15.0) *|I(INV1:IN INV1 IN I 0.0PF 30.0 15.0) C6 DF1:C VSS 0.208719PF C7 INV1:IN VSS 0.783500PF R24 DF1:C INV1:IN 1.80833E-01 *|NET OUT 0.148478PF *|S(OUT:1 45.0 15.0) *|P(OUT O 0.0PF 50.0 5.0) *|I(INV1:OUT INV1 OUT O 0.0PF 40.0 15.0) C8 INV1:OUT VSS 0.147069PF C9 OUT:1 VSS 0.632813PF C10 OUT VSS 0.776250PF R25 INV1:OUT OUT:1 3.11000E00 R26 OUT:1 OUT 3.03333E00 * Description of Instances XDF1 DF1:A DF1:B DF1:C DFF XINV1 INV1:IN INV1:OUT INV .ENDS .END 332 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Overview of SPEF Files The Standard Parasitics Exchange Format (SPEF) file structure is described in IEEE standard IEEE-1481. For information about how to obtain the complete SPEC (IEEE-1481) specification, or any other documents from IEEE, see: http://www.ieee.org/products/onlinepubs/stand/standards.html SPEF File Structure The IEEE-1481 specification requires the following file structure in a SPEF file. Parameters in [brackets] are optional: HSPICE® RF User Guide Z-2007.03 333 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation SPEF_file : := *SPEF version *DESIGN design_name *DATE date *VENDOR vendor *PROGRAM program_name *VERSION program_version *DESIGN_FLOW flow_type {flow_type} *DIVIDER divider *DELIMITER delimiter *BUS_DELIMITER bus_prefix bus_suffix *T_UNIT time_unit NS|PS *C_UNIT capacitance_unit FF|PF *R_UNIT resistance_unit OHM|KOHM *L_UNIT inductance_unit HENRY|MH|UH [*NAME_MAP name_index name_id|bit|path|name|physical_ref] [*POWER_NETS logical_power_net physical_power_net ...] [*GROUND_NETS ground_net ...] [*PORTS logical_port I|B|O *C coordinate ... *L par_value *S rising_slew falling_slew [low_threshold high_threshold] *D cell_type] [*PHYSICAL_PORTS [physical_instance delimiter] physical_port I|B|O *C coordinate ... *L par_value *S rising_slew falling_slew [low_threshold high_threshold] *D cell_type] [*DEFINE logical_instance design_name | *PDEFINE physical_instance design_name] *D_NET net_path total_capacitance [*V routing_confidence] [*CONN *P [logical_instance delimiter] logical_port|physical_port I|B|O *C coordinate ... *L par_value *S rising_slew falling_slew [low_threshold high_threshold] *D cell_type | *I [physical_instance delimiter] logical_pin|physical_node I|B|O 334 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation *C coordinate ... *L par_value *S rising_slew falling_slew [low_threshold high_threshold] *D cell_type *N net_name delimiter net_number coordinate [*CAP cap_id node1 [node2] capacitance] [*RES res_id node1 node2 resistance] [*INDUC induc_id node1 node2 inductance] *END Table 26 SPEF Parameters Parameter Definition *SPEF Specifies that the file is in SPEF format. {version} Version number of the SPEF specification, such as “IEEE 14811998”. * Words that start with an asterisk (*) are keywords. | Or. For example, NS|PS means choose either nanoseconds or picoseconds as the time units. design_name Name of your circuit design. date Date and time when a parasitic extraction tool (such as Star-RCXT) generated the SPEF file. vendor Name of the vendor (such as Synopsys) whose tools you used to generate the SPEF file (optional). program_name Name of the program (such as Star-RCXT) that generated the SPEF file. program_version Version number of the program that generated the SPEF file. HSPICE® RF User Guide Z-2007.03 335 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 26 SPEF Parameters (Continued) Parameter Definition flow_type One or more of the following flow types: ■ ■ ■ ■ ■ ■ ■ 336 EXTERNAL_LOADS: The SPEF file defines all external loads (if any). If you do not specify this flow type, then some or all external loads are not defined in this SPEF file. If HSPICE RF cannot find external load data outside the SPEF file, it reports an error. EXTERNAL_SLEWS: The SPEF file defines all external slews (if any). If you do not specify this flow type, then some or all external slews are not defined in this SPEF file. If HSPICE RF cannot find external slew data outside the SPEF file, it reports an error. FULL_CONNECTIVITY: A SPEF file defines all net connectivity. If you do not specify this flow type, then some or all net connectivity is not defined in this SPEF file. If HSPICE RF cannot find connectivity data outside the SPEF file, it issues an error. This flow does not look for presence or absence of power and ground nets, or any other nets that do not correspond to the logical netlist. If a SPEC file includes FULL_CONNECTIVITY and MISSING_NETS, HSPICE RF reports an error. MISSING_NETS: If any logical nets are not defined in the netlist, HSPICE RF merges missing parasitic data from another source. If it does not find another source, HSPICE RF rereads the netlist and estimates the missing parasitics. This flow does not look for presence or absence of power and ground nets, or any other nets that do not correspond to the logical netlist. If you use FULL_CONNECTIVITY and MISSING_NETS in the same SPEF file, HSPICE RF reports an error. NETLIST_TYPE_VERILOG, NETLIST_TYPE_VHDL87, NETLIST_TYPE_VHDL93, or NETLIST_TYPE_EDIF: Specifies the type of naming conventions used in the SPEF file. If you specify more than one format in one SPEF file, HSPICE RF reports an error. ROUTING_CONFIDENCE positive_integer: Specifies a default routing confidence value for all nets in the SPEF file. ROUTING_CONFIDENCE_ENTRY positive_integer character_string: Specifies one or more characters that represent additional routing confidence values, which you can assign to nets in the SPEF file. HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 26 SPEF Parameters (Continued) Parameter Definition flow_type (continued) ■ ■ ■ divider NAME_SCOPE LOCAL|FLAT: Specifies whether paths in the SPEF file are LOCAL (relative to the current SPEF file) or FLAT (relative to the top level of your circuit design). SLEW_THRESHOLDS low high: Specifies low and high default input slew thresholds for your circuit design as a percentage of the voltage level for the input pin. PIN_CAP NONE|INPUT_OUTPUT|INPUT_ONLY: Specifies the type of pin capacitance to include when calculating the total capacitance for all nets in the SPEF file, either no capacitance, all input and output capacitances, or only input capacitances. Character used to divide levels of hierarchy in a circuit path name. Must be one of the following characters: . / : | For example, X1/X2 means that X2 is a subcircuit of the X1 circuit. delimiter Character used to separate the name of an instance and a pin in a concatenated instance pin name. Must be one of these characters: ./:| bus_prefix bus_suffix Delimiter characters that precede and follow a bus bit or an arrayed instance number. If these characters are not matching pairs, HSPICE RF reports an error. Valid bus delimiter prefix and suffix character pairs are brackets “[ ]”, braces “{ }”, parentheses “( )”, or angle brackets “< >”> time_unit A positive number. For example, 10 PS means use time units of 10 picoseconds. 5 NS means use time units of 5 nanoseconds. capacitance_unit A positive number. For example, 10 PF means capacitance units of 10 picofarads. 5 FF means use capacitance units of 5 femtoseconds. resistance_unit Positive number. For example, 10 OHM sets resistance units to 10 ohms. 5 KOHM sets resistance units to 5 kilo ohms. inductance_unit A positive number. For example, 10 HENRY means use inductance units of 10 henries. 5 MH means use inductance units of 5 millihenries. 2 UH means use inductance units of 2 micro-henries. name_index Name used throughout a SPEF file. To reduce file space, you can map other names to this name. HSPICE® RF User Guide Z-2007.03 337 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 26 SPEF Parameters (Continued) Parameter Definition name_id|bit|path|name| physical_ref A name identifier, bit, path, name, or physical reference to map to the name_index. logical_power_net Logical path (or logical path index) to a power net. physical_power_net Physical path (or physical path index) to a power net. You can specify multiple logical_power_net physical_power_net pairs. ground_net Name of a net to use as a ground net. You can specify multiple ground net names. logical_port Logical name of an input, output, or bidirectional port. coordinate Geometric location of a logical or physical port. par_value Either a single float value, or a triplet in float:float:float form. rising_slew Rising slew of the waveform for the port. T_UNIT defines the time unit for the waveform. falling_slew Rising slew of the waveform for the port. T_UNIT defines the time unit for the waveform. low_threshold Low voltage threshold as a percentage of the port’s input voltage. Can bed one float value or a triplet in float:float:float form. high_threshold High voltage threshold as a percentage of the input voltage for the port. Either a single float value or a triplet in float:float:float form. cell_type Type of cell that drives the port. If you do not know the cell type, use the reserved word UNKNOWN_DRIVER as the cell type. physical_port Physical name of an input, output, or bidirectional port. logical_instance Logical name of a subcircuit in your design_name circuit design. You can specify more than one logical_instance. Whenever you specify a logical instance name, you must set NAME_SCOPE to FLAT. If you connect a logical net to a physical port, HSPICE RF reports an error. 338 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 26 SPEF Parameters (Continued) Parameter Definition physical_instance Physical name of a subcircuit in your design_name circuit design. You can specify more than one physical_instance. Whenever you specify a physical instance name, you must set NAME_SCOPE to FLAT. If you connect a physical net to a logical port, HSPICE RF reports an error. routing_confidence One of the following positive integers: ■ ■ ■ ■ ■ ■ ■ ■ ■ ■ 10: Statistical wire load model. 20: Physical wire load model. 30: Physical partitions with locations, no cell placement. 40: Estimated cell placement with Steiner tree-based route. 50: Estimated cell placement with global route. 60: Final cell placement with Steiner route. 70: Final cell placement with global route. 80: Final cell placement, final route, 2d extraction. 90: Final cell placement, final route, 2.5d extraction. 100: Final cell placement, final route, 3d extraction. logical_pin Logical name of a pin. physical_node Physical name of a node. net_name Name of a net in a circuit or subcircuit. cap_id Unique identifier for capacitance between two specific nodes. res_id Unique identifier for resistance between two specific nodes. induc_id Unique identifier for inductance between two specific nodes. node1 First of two nodes, between which you are specifying a capacitance, resistance, or inductance value. node2 Second of two nodes, between which you are specifying a capacitance, resistance, or inductance value. For a capacitance value, if you do not specify a second node name, HSPICE RF assumes that the second node is ground. HSPICE® RF User Guide Z-2007.03 339 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation Table 26 SPEF Parameters (Continued) Parameter Definition capacitance Specifies the capacitance value assigned to a cap_id identifier. capacitance_unit defines the units of capacitance. For example, if you set capacitance to 5 and capacitance_unit to 10 PF, then the actual capacitance value is 50 picoFarads. resistance Specifies the resistance value assigned to a res_id identifier. resistance_unit defines the units of resistance. For example, if you set resistance to 5 and resistance_unit to 5 KOHM, then the actual resistance value is 25 kilo ohms. inductance Specifies the resistance value assigned to an induc_id identifier. inductance_unit defines the units of inductance. For example, if you set inductance to 6 and inductance_unit to 2 UH, then the actual inductance value is 12 microhenries. SPEF File Example *SPEF "IEEE 1481-1998" *DESIGN "My_design" *DATE "11:26:34 Friday June 28, 2002" *VENDOR "Synopsys, Inc." *PROGRAM "Star-RCXT" *VERSION "2002.2." *DESIGN_FLOW "EXTERNAL_LOADS" "EXTERNAL_SLEWS" "MISSING_NETS" *DIVIDER / *DELIMITER : *BUS_DELIMITER [ ] *T_UNIT 1 NS *C_UNIT 1 PF *R_UNIT 1 OHM *L_UNIT 1 HENRY *POWER_NETS VDD *GND_NETS VSS *PORTS CONTROL O *L 30 *S 0 0 FARLOAD O *L 30 *S 0 0 INVX1FNTC_IN I *L 30 *S 5 5 NEARLOAD O *L 30 *S 0 0 TREE O *L 30 *S 0 0 340 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation If you use triplet format, the above section would look like this: *PORTS CONTROL O *L 30:30:30 *S 0:0:0 0:0:0 FARLOAD O *L 30:30:30 *S 0:0:0 0:0:0 INVX1FNTC_IN I *L 30:30:30 *S 5:5:5 5:5:5 NEARLOAD O *L 30:30:30 *S 0:0:0 0:0:0 TREE O *L 30:30:30 *S 0:0:0 0:0:0 This triplet formatting principle applies to the rest of this example. HSPICE® RF User Guide Z-2007.03 341 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation *D_NET INVX1FNTC_IN 0.033 *CONN *P INVX1FNTC_IN I *I FL_1281:A *L 0.033 *END *D_NET INVX1FNTC 2.033341 *CONN *I FL_1281:X *I I1184:A I *I FL_1000:A *I NL_1000:A *I TR_1000:A O *L 0.0 *L 0.343 I *L 0.343 I *L 0.343 I *L 0.343 *CAP 216 FL_1000:A 0.346393 217 I1184:A 0.344053 218 INVX1FNTC_IN 0 219 INVX1FNTC_IN:10 0.154198 220 INVX1FNTC_IN:11 0.117827 221 INVX1FNTC_IN:12 0.463063 222 INVX1FNTC_IN:13 0.0384381 223 INVX1FNTC_IN:14 0.00246845 224 INVX1FNTC_IN:15 0.00350198 225 INVX1FNTC_IN:16 0.00226712 226 INVX1FNTC_IN:17 0.0426184 227 INVX1FNTC_IN:18 0.0209701 228 INVX1FNTC_IN:2 0.0699292 229 INVX1FNTC_IN:20 0.019987 230 INVX1FNTC_IN:21 0.0110279 231 INVX1FNTC_IN:24 0.0192603 232 INVX1FNTC_IN:25 0.0141824 233 INVX1FNTC_IN:3 0.0520437 234 INVX1FNTC_IN:4 0.0527105 235 INVX1FNTC_IN:5 0.1184749 236 INVX1FNTC_IN:6 0.0468458 237 INVX1FNTC_IN:7 0.0391578 238 INVX1FNTC_IN:8 0.0113856 239 INVX1FNTC_IN:9 0.0142528 240 NL_1000:A 0.344804 241 TR_000:A 0.34506 *RES 152 INVX1FNTC_IN INVX1FNTC_IN:18 8.39117 153 INVX1FNTC_IN INVX1FNTC_IN:5 25.1397 154 INVX1FNTC_IN:11 INVX1FNTC_IN:20 4.59517 155 INVX1FNTC_IN:12 INVX1FNTC_IN:13 3.688 156 INVX1FNTC_IN:13 INVX1FNTC_IN:17 25.102 342 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Post-Layout Back-Annotation 157 158 159 160 161 162 163 164 165 166 167 168 169 170 171 172 173 174 175 176 INVX1FNTC_IN:14 INVX1FNTC_IN:16 0.0856444 INVX1FNTC_IN:14 NL_1000:A 0.804 INVX1FNTC_IN:15 INVX1FNTC_IN:16 1.73764 INVX1FNTC_IN:15 INVX1FNTC_IN:24 0.307175 INVX1FNTC_IN:17 INVX1FNTC_IN:25 5.65517 INVX1FNTC_IN:18 FL_1000:A 1/36317 INVX1FNTC_IN:2 INVX1FNTC_IN:4 6.95371 INVX1FNTC_IN:2 INVX1FNTC_IN:5 50.9942 INVX1FNTC_IN: INVX1FNTC_IN:21 4.71035 INVX1FNTC_IN: I1184:A 0.403175 INVX1FNTC_IN: TR_1000:A 0.923175 INVX1FNTC_IN: INVX1FNTC_IN:12 31.7256 INVX1FNTC_IN: INVX1FNTC_IN:4 11.9254 INVX1FNTC_IN: INVX1FNTC_IN:7 25.3618 INVX1FNTC_IN: INVX1FNTC_IN:6 23.3057 INVX1FNTC_IN: INVX1FNTC_IN:24 8.64717 INVX1FNTC_IN: INVX1FNTC_IN:8 7.46529 INVX1FNTC_IN: INVX1FNTC_IN:10 2.04729 INVX1FNTC_IN: INVX1FNTC_IN:10 10.8533 INVX1FNTC_IN: INVX1FNTC_IN:11 1.05164 *END *D_NET NE_794 1.98538 *CONN *I NL_1039:X O *L 0 *D INVX *I NL_2039:A I *L 0.343 *I NL_1040:A I *L 0.343 *CAP 3387 3388 3389 3390 3391 3392 3393 3394 3395 3396 3397 3398 3399 3400 3401 3402 3403 NE_794 0 NE_794:1 0.0792492 NE_794:10 0.0789158 NE_794:11 0.0789991 NE_794:12 0.0789991 NE_794:13 0.0792992 NE_794:14 0.00093352 NE_794:15 0.00063346 NE_794:16 0.0792992 NE_794:17 0.80116 NE_794:18 0.80116 NE_794:19 0.00125452 NE_794:2 0.0789158 NE_794:20 0.00336991 NE_794:21 0.00668512 NE_794:23 0.00294932 NE_794:25 0.00259882 HSPICE® RF User Guide Z-2007.03 343 Chapter 13: Post-Layout Analysis Linear Acceleration 3404 3405 3406 3407 3408 3409 3410 3411 3412 3413 3414 NE_794:26 0.00184653 NE_794:3 0.0789158 NE_794:4 0.0796826 NE_794:5 0.0796826 NE_794:6 0.0789991 NE_794:7 0.0789991 NE_794:8 0.0793992 NE_794:9 0.0789158 NL_1039:X 0.00871972 NL_1040:A 0.344453 NL_2039:A 0.343427 *RES 2879 2880 2881 2882 2883 2884 2885 2886 2887 2888 2889 2890 2891 2892 2893 2894 2895 2896 2897 2898 2899 2900 2901 2902 2903 2904 NE_794:1 NE_794:13 66.1953 NE_794:1 NE_794:2 0.311289 NE_794:11 NE_794:12 0.311289 NE_794:13 NE_794:14 0.353289 NE_794:14 NE_794:19 0.365644 NE_794:15 NE_794:16 0.227289 NE_794:15 NE_794:20 0.239644 NE_794:17 NE_794:18 0.14 NE_794:19 NE_794:21 0.0511746 NE_794:2 NE_794:9 65.9153 NE_794:20 NE_794:23 1.15117 NE_794:21 NL_1039:X 3.01917 NE_794:25 NE_794:26 0.166349 NE_794:26 NL_1040:A 0.651175 NE_794:3 NE_794:10 65.9153 NE_794:3 NE_794:4 0.311289 NE_794:4 NE_794:17 66.5437 NE_794:5 NE_794:18 66.5437 NE_794:5 NE_794:6 0.311289 NE_794:6 NE_794:11 65.98853 NE_794:7 NE_794:12 65.9853 NE_794:7 NE_794:8 0.311289 NE_794:8 NE_794:16 66.3213 NE_794:9 NE_794:10 0.311289 NL_1039:X NE_794:25 1.00317 NL_2039:A NE_794:23 0.171175 *END Linear Acceleration Linear acceleration, by using the SIM_LA option, accelerates the simulation of circuits that include large linear RC networks. To achieve this acceleration, 344 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Linear Acceleration HSPICE RF reduces all matrices that represent RC networks. The result is a smaller matrix that maintains the original port behavior, yet achieves significant savings in memory and computation. Thus, the SIM_LA option is ideal for circuits with large numbers of resistors and capacitors, such as clock trees, power lines, or substrate networks. In general, the RC elements are separated into their own network. The nodes shared by both main circuit elements (including .PRINT, .PROBE, and .MEASURE statements), and RC elements. are the port nodes of the RC network,. All other RC nodes are internal nodes. The currents flowing into the port nodes are a frequency-dependent function of the voltages at those nodes. The multiport admittance of a network represents this relationship. ■ The SIM_LA option formulates matrices to represent multiport admittance. ■ Then, to eliminate as many internal nodes as possible, it reduces the size of these matrices, while preserving the admittance, otherwise known as port node behavior. ■ The amount of reduction depends on the f0 upper frequency, the threshold frequency where SIM_LA preserves the admittance. This is shown graphically in Figure 26. Multiport Admittance vs. Frequency nce itta m d a ual approx act admittance Figure 26 f0 frequency The SIM_LA option is very effective for post-layout simulation, because of the volume of parasitics. For frequencies below f0, the approx signal matches that of the original admittance. Above f0, the two waveforms diverge, but presumably the higher frequencies are not of interest. The lower the f0 frequency, the greater the amount of reduction. For the syntax and description of this control option, see .OPTION SIM_LA in the HSPICE and HSPICE RF Command Reference. HSPICE® RF User Guide Z-2007.03 345 Chapter 13: Post-Layout Analysis Linear Acceleration You can choose one of two algorithms, explained in the following sections: ■ PACT Algorithm ■ PI Algorithm PACT Algorithm The PACT (Pole Analysis via Congruence Transforms) algorithm reduces the RC networks in a well-conditioned manner, while preserving network stability. ■ The transform preserves the first two moments of admittance at DC (slope and offset), so that DC behavior is correct (see Figure 27). ■ The algorithm preserves enough low-frequency poles from the original network to maintain the circuit behavior up to a specified maximum frequency f0, within the specified tolerance. This approach is the most accurate of the two algorithms, and is the default. PACT Algorithm ed erv s re tp e s off nd ce a tan e t i p dm slo al a u t ac admittance Figure 27 PACT: poles added f0 frequency PI Algorithm This algorithm creates a pi model of the RC network. ■ 346 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 HSPICE® RF User Guide Z-2007.03 Chapter 13: Post-Layout Analysis Linear Acceleration The result resembles the Greek letter pi. ■ For a general multiport, SIM_LA preserves the DC admittance between the ports, and the total capacitance that connects the ports to ground. All floating capacitances are lumped to ground. Linear Acceleration Control Options Summary In addition to .OPTION SIM_LA, other options are available to control the maximum resistance and minimum capacitance values to preserve, and to limit the operating parameters of the PACT algorithm. Table 27 contains a summary of these control options. For the syntax and descriptions of these control options, see the respective section in the HSPICE and HSPICE RF Command Reference. Table 27 PACT Options Syntax Description .OPTION SIM_LA=PACT | PI Activates linear matrix reduction and selects between two methods. .OPTION SIM_LA_FREQ=<value> Upper frequency where you need accuracy preserved. value is the upper frequency for which the PACT algorithm preserves accuracy. If value is 0, PACT drops all capacitors, because only DC is of interest. The maximum frequency required for accurate reduction depends on both the technology of the circuit and the time scale of interest. In general, the faster the circuit, the higher the maximum frequency. The default is 1GHz. .OPTION SIM_LA_MAXR=<value> Maximum resistance for linear matrix reduction. value is the maximum resistance preserved in the reduction. SIM_LA assumes that any resistor greater than value has an infinite resistance, and drops the resistor after reduction finishes. The default is 1e15 ohms. HSPICE® RF User Guide Z-2007.03 347 Chapter 13: Post-Layout Analysis Linear Acceleration Table 27 PACT Options (Continued) Syntax Description .OPTION SIM_LA_MINC=<value> Minimum capacitance for linear matrix reduction. value is the minimum capacitance preserved in the reduction. After reduction completes, SIM_LA lumps any capacitor smaller than value to ground. The default is 1e-16 farads. .OPTION SIM_LA_MINMODE= ON|OFF Reduces the number of nodes instead of the number of elements. .OPTION SIM_LA_TIME=<value> Minimum time for which accuracy must be preserved. value is the minimum switching time for which the PACT algorithm preserves accuracy. HSPICE RF does not accurately represent waveforms that occur more rapidly than this time. SIM_LA_TIME is simply the dual of SIM_LA_FREQ. The default is equivalent to setting LA_FREQ=1 GHz. The default is 1ns. .OPTION SIM_LA_TOL=<value> Error tolerance for the PACT algorithm. value is the error tolerance for the PACT algorithm, is between 0.0 and 1.0. The default is 0.05. Example In this example, the circuit has a typical risetime of 1ns. Set the maximum frequency to 1 GHz, or set the minimum switching time to 1ns. .OPTION SIM_LA_FREQ = 1GHz -or.OPTION SIM_LA_TIME = 1ns However, if spikes occur in 0.1ns, HSPICE will not accurately simulate them. To capture the behavior of the spikes, use: .OPTION SIM_LA_FREQ = 10GHz -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. 348 HSPICE® RF User Guide Z-2007.03 14 Statistical and Monte Carlo Analysis 14 Describes the features available in HSPICE RF for statistical analysis. Overview Described in this chapter are the features available in HSPICE RF for statistical analysis. These features are supported for HSPICE RF and differ from the enhanced statistical analysis features available for HSPICE (described in the HSPICE Simulation and Analysis User Guide.) The following subjects are described in this chapter: ■ Application of Statistical Analysis ■ Analytical Model Types ■ Simulating Circuit and Model Temperatures ■ Worst Case Analysis ■ Monte Carlo Analysis ■ Worst Case and Monte Carlo Sweep Example ■ Simulating the Effects of Global and Local Variations with Monte Carlo Application of Statistical Analysis When you design an electrical circuit, it must meet tolerances for the specific manufacturing process. The electrical yield is the number of parts that meet the electrical test specifications. Overall process efficiency requires maximum yield. To analyze and optimize the yield, HSPICE RF supports statistical techniques and observes the effects of variations in element and model parameters. HSPICE® RF User Guide Z-2007.03 349 Chapter 14: Statistical and Monte Carlo Analysis Analytical Model Types Analytical Model Types To model parametric and statistical variation in circuit behavior, use: ■ .PARAM statement to investigate the performance of a circuit as you change circuit parameters. For details about the .PARAM statement, see the .PARAM statement in the HSPICE and HSPICE RF Command Reference. ■ Temperature variation analysis to vary the circuit and component temperatures, and compare the circuit responses. You can study the temperature-dependent effects of the circuit, in detail. ■ Monte Carlo analysis when you know the statistical standard deviations of component values to center a design. This provides maximum process yield, and determines component tolerances. ■ Worst-case corner analysis when you know the component value limit to automate quality assurance for: ■ • basic circuit function • process extremes • quick estimation of speed and power tradeoffs • best-case and worst-case model selection • parameter corners • library files Data-driven analysis for cell characterization, response surface, or Taguchi analysis. See “Performing Digital Cell Characterization” in the HSPICE Applications Manual. Automates characterization of cells and calculates the coefficient of polynomial delay for timing simulation. You can simultaneously vary any number of parameters and perform an unlimited number of analyses. This analysis uses an ASCII file format so HSPICE RF can automatically generate parameter values. This analysis can replace hundreds or thousands of HSPICE RF simulation runs. Use yield analyses to modify: 350 ■ DC operating points ■ DC sweeps ■ AC sweeps ■ Transient analysis. HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Simulating Circuit and Model Temperatures CosmosScope can generate scatter plots from the operating point analysis or a family of curve plots for DC, AC, and transient analysis. Use .MEASURE statements to save results for delay times, power, or any other characteristic extracted in a .MEASURE statement. HSPICE RF generates a table of results in an .mt# file in ASCII format. You can analyze the numbers directly or read this file into CosmosScope to view the distributions. Also, if you use .MEASURE statements in a Monte Carlo or data-driven analysis, then the HSPICE RF output file includes the following statistical results in the listing: Mean x 1 + x 2 + …+ x n -------------------------------------N Variance Sigma ( x 1 – Mean ) 2 + …x ( n – Mean ) 2 ---------------------------------------------------------------------------N–1 Variance Average Deviation x 1 – Mean + …+ x n – Mean ------------------------------------------------------------------------N–1 Simulating Circuit and Model Temperatures Temperature affects all electrical circuits. Figure 28 shows the key temperature parameters associated with circuit simulation: ■ Model reference temperature – you can model different models at different temperatures. Each model has a TREF (temperature reference) parameter. ■ Element junction temperature – each resistor, transistor, or other element generates heat so an element is hotter than the ambient temperature. ■ 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. HSPICE® RF User Guide Z-2007.03 351 Chapter 14: Statistical and Monte Carlo Analysis Simulating Circuit and Model Temperatures Figure 28 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 RF calculates temperatures as differences from the ambient temperature: Equation 68 Tambient + Δsystem + Δpart + Δjunction = Tjunction Equation 69 Ids = f ( Tjunction, Tmodel ) Every element includes a DTEMP keyword, which defines the difference between junction and ambient temperature. Example The following example uses DTEMP in a MOSFET element statement: M1 drain gate source bulk Model_name W=10u L=1u DTEMP=+20 Temperature Analysis You can specify three temperatures: 352 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Simulating Circuit and Model 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 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 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 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 RF uses the difference between the circuit simulation temperature, and the TNOM reference temperature. Elements and models within a circuit can operate at different temperatures. For example, a high-speed input/output buffer that switches at 50 MHz is much hotter than a low-drive NAND gate that switches at 1 MHz). To simulate this temperature difference, specify both an element temperature parameter (DTEMP), and a model reference parameter (TREF). If you specify DTEMP in an element statement, the element temperature for the simulation is: element temperature=circuit temperature + DTEMP Specify the DTEMP value in the element statement (resistor, capacitor, inductor, diode, BJT, JFET, or MOSFET statement), or in a subcircuit element. Assign a parameter to DTEMP, then use the .DC statement to sweep the parameter. The DTEMP value defaults to zero. 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). HSPICE® RF User Guide Z-2007.03 353 Chapter 14: Statistical and Monte Carlo Analysis Worst Case Analysis .TEMP Statement To specify the temperature of a circuit for a HSPICE RF simulation, use the .TEMP statement. Worst Case Analysis Circuit designers often use worst-case analysis when designing and analyzing MOS and BJT IC circuits. To simulate the worst case, set all variables to their 2or 3-sigma worst-case values. Because several independent variables rarely attain their worst-case values simultaneously, this technique tends to be overly pessimistic and can lead to over-designing the circuit. However, this analysis is useful as a fast check. Model Skew Parameters The HSPICE RF device models include physically-measurable model parameters. The circuit simulator uses parameter variations to predict how an actual circuit responds to extremes in the manufacturing process. Physicallymeasurable model parameters are called skew parameters, because they skew from a statistical mean to obtain predicted performance variations. Examples of skew parameters are the difference between the drawn and physical dimension of metal, postillion, or active layers, on an integrated circuit. Generally, you specify skew parameters independently of each other, so you can use combinations of skew parameters to represent worst cases. Typical skew parameters for CMOS technology include: ■ XL – polysilicon CD (critical dimension of the poly layer, representing the difference between drawn and actual size). ■ XWn, XWp – active CD (critical dimension of the active layer, representing the difference between drawn and actual size). ■ TOX – thickness of the gate oxide. ■ 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 RF device models. The DELVTO parameter shifts the threshold value. HSPICE 354 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case Analysis RF adds this value to VTO for the Level 3 model, and adds or subtracts it from VFB0 for the BSIM model. Table 28 shows whether HSPICE RF adds or subtracts deviations from the average. Table 28 Sigma Deviations Type Parameter Slow Fast NMOS XL + - RSH + - DELVTO + - TOX + - XW - + XL + - RSH + - DELVTO - + TOX + - XW - + PMOS HSPICE RF selects skew parameters based on the available historical data that it collects either during fabrication or electrical test. For example, HSPICE RF collects the XL skew parameter for poly CD during fabrication. This parameter is usually the most important skew parameter for a MOS process. Figure 29 is an example of data that historical records produce. HSPICE® RF User Guide Z-2007.03 355 Chapter 14: Statistical and Monte Carlo Analysis Worst Case Analysis Figure 29 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 Figure 30 shows how to create a worst-case corners library file for a CMOS process model. 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 30 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 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 356 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case Analysis 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. 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® RF User Guide Z-2007.03 357 Chapter 14: Statistical and Monte Carlo Analysis Worst Case Analysis Skew File Interface to Device Models Skew parameters are model parameters for transistor models or passive components. A typical device model set includes: ■ MOSFET models for all device sizes by using an automatic model selector. ■ RC wire models for polysilicon, metal1, and metal2 layers in the drawn dimension. Models include temperature coefficients and fringe capacitance. ■ Single-diode and distributed-diode models for N+, P+, and well (includes temperature, leakage, and capacitance based on the drawn dimension). ■ BJT models for parasitic bipolar transistors. You can also use these for any special BJTs, such as a BiCMOS for ECL BJT process (includes current and capacitance as a function of temperature). ■ Metal1 and metal2 transmission line models for long metal lines. ■ Models must accept elements. Sizes are based on a drawn dimension. If you draw a cell at 2μ dimension and shrink it to 1μ, the physical size is 0.9μ. The effective electrical size is 0.8μ. Account for the four dimension levels: • drawn size • shrunken size • physical size • electrical size Most simulator models scale directly from drawn to electrical size. HSPICE MOS models support all four size levels as in Figure 31. 358 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Figure 31 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 uses a random number generator to create the following types of functions. ■ ■ ■ Gaussian parameter distribution • Relative variation—variation is a ratio of the average. • Absolute variation—adds variation to the average. • Bimodal–multiplies distribution to statistically reduce nominal parameters. Uniform parameter distribution • Relative variation—variation is a ratio of the average. • Absolute variation—adds variation to the average. • Bimodal–multiplies distribution to statistically reduce nominal parameters. Random limit parameter distribution • Absolute variation—adds variation to the average. • Monte Carlo analysis randomly selects the min or max variation. HSPICE® RF User Guide Z-2007.03 359 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis The value of the MONTE analysis keyword determines how many times to perform operating point, DC sweep, AC sweep, or transient analysis. Figure 32 Monte Carlo Distribution Uniform Distribution Gaussian Distribution Population Population Abs variation Abs variation 3 Sigma Nom_value Nom_value Rel_variation=Abs_variation/Nom_value Monte Carlo Setup To set up a Monte Carlo analysis, use the following HSPICE statements: ■ .PARAM statement—sets a model or element parameter to a Gaussian, Uniform, or Limit function distribution. ■ .DC, .AC, or .TRAN analysis—enables MONTE. ■ .MEASURE statement—calculates the output mean, variance, sigma, and standard deviation. ■ .MODEL statement—sets model parameters to a Gaussian, Uniform, or Limit function distribution. Select the type of analysis to run, such as operating point, DC sweep, AC sweep, or TRAN sweep. Operating Point .DC MONTE=<firstrun=num1> -or.DC MONTE=list <(> <num1:num2> <num3> <num5:num6> <num7> <)> DC Sweep .DC vin 1 5 0.25 sweep MONTE=val <firstrun=num1> 360 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis -or.DC vin 1 5 0.25 sweep MONTE=list<(> <num1:num2> <num3> + <num5:num6> <num7> <)> AC Sweep .AC dec 10 100 1meg sweep MONTE=val <firstrun=num1> -or.AC dec 10 100 1meg sweep MONTE=list<(> <num1:num2> + <num3> <num5:num6> <num7> <)> TRAN Sweep .TRAN 1n 10n sweep MONTE=val <firstrun=num1> -or.TRAN 1n 10n sweep MONTE=list<(> <num1:num2> <num3> + <num5:num6> <num7> <)> The val value specifies the number of Monte Carlo iterations to perform. A reasonable number is 30. The statistical significance of 30 iterations is quite high. If the circuit operates correctly for all 30 iterations, there is a 99% probability that over 80% of all possible component values operate correctly. The relative error of a quantity, determined through Monte Carlo analysis, is proportional to val-1/2. The firstrun values specify the desired number of iterations. HSPICE RF 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 RF runs only a the one specified point. Example 1 In this example, HSPICE RF 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 RF run only at that single point. Example 1 In this example, HSPICE RF 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. HSPICE® RF User Guide Z-2007.03 361 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis .tran 1n 10n sweep monte=list(10 20:30 40 46:72) Monte Carlo Output ■ .MEASURE statements are the most convenient way to summarize the results. ■ .PRINT statements generate tabular results, and print the values of all Monte Carlo parameters. ■ .MCBRIEF determines the output types of the random parameters during Monte Carlo analysis to improve output performance. ■ If one iteration is out of specification, you can obtain the component values from the tabular listing. A detailed resimulation of that iteration might help identify the problem. ■ AvanWaves superimposes all iterations as a single plot so you can analyze each iteration individually. .PARAM Distribution Function This section describes how to use assign a .PARAM parameter in Monte Carlo analysis. For a general description of the .PARAM statement, see the .PARAM command in the HSPICE and HSPICE RF 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 RF 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>) 362 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis .PARAM xx=LIMIT(nominal_val, abs_variation) Argument Description xx Distribution function calculates the value of this parameter. UNIF Uniform distribution function by using relative variation. AUNIF Uniform distribution function by using absolute variation. GAUSS Gaussian distribution function by using relative variation. AGAUSS Gaussian distribution function by using absolute variation LIMIT Random-limit distribution function by using absolute variation. Adds +/- abs_variation to nominal_val based on whether the random outcome of a -1 to 1 distribution is greater than or less than 0. nominal_val Nominal value in Monte Carlo analysis and default value in all other analyses. abs_variation AUNIF and AGAUSS vary the nominal_val by +/- abs_variation. rel_variation UNIF and GAUSS vary the nominal_val by +/- (nominal_val ⋅ rel_variation). sigma Specifies abs_variation or rel_variation at the sigma level. For example, if sigma=3, then the standard deviation is abs_variation divided by 3. multiplier If you do not specify a multiplier, the default is 1. HSPICE RF recalculates many times and saves the largest deviation. The resulting parameter value might be greater than or less than nominal_val. The resulting distribution is bimodal. Example 1 In this example, each R has an unique variation. .param mc_var=agauss(0,1,3) .param val='1000*(1+mc_var)' v_vin vin 0 dc=1 ac=.1 r1 vin 0 '1000*(1+mc_var)' r2 vin 0 '1000*(1+mc_var)' HSPICE® RF User Guide Z-2007.03 $ +/- 20% swing 363 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Example 2 In this example, each R has an identical variation. .param mc_var=agauss(0,1,3) .param val='1+mc_var' v_vin vin 0 dc=1 ac=.1 r1 vin 0 '1000*val' r2 vin 0 '1000*val' $ +/- 20% swing Example 3 In this example, local variations to an instance parameter are applied by assigning randomly-generated variations directly to each instance parameter. Each resistor r1 through r3 receives randomly different resistance values during each Monte Carlo run. .param r1 1 2 r2 3 4 r3 5 6 r_local=agauss(...) r=r_local r=r_local r=r_local Example 4 In this example, global variations to an instance parameter are applied by assigning the variation to an intermediate parameter before assigning it to each instance parameter. Each resistor r1 through r3 receives the same random resistance value during each Monte Carlo run. .param .param r1 1 2 r2 3 4 r3 5 6 r_random=agauss(...) r_global=r_random r=r_global r=r_global r=r_global Monte Carlo Parameter Distribution Each time you use a parameter, Monte Carlo calculates a new random variable. ■ If you do not specify a Monte Carlo distribution, then HSPICE RF assumes the nominal value. ■ If you specify a Monte Carlo distribution for only one analysis, HSPICE RF uses the nominal value for all other analyses. You can assign a Monte Carlo distribution to all elements that share a common model. The actual element value varies according to the element distribution. If you assign a Monte Carlo distribution to a model keyword, then all elements 364 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis 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 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 33 119.182 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® RF User Guide Z-2007.03 365 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Figure 34 115.0 Gaussian Functions MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS May 15 2003 11:41:23 MONT1_SV RGAUSS_1 110.0 VOLT [LIN] 105.0 100.0 95.0 90.0 MONT1_SV RGAUSS_1 118.375 110.0 100.0 90.0 80.9998 1.0 10.0 20.0 30.0 40.0 50.0 60.0 MONTE CARLO [LIN] 366 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Figure 35 Limit Functions MONT1.SP TEST OF MONTE CARLO, GAUSSIAN, UNIFORM, AND LIMIT FUNCTIONS May 15 2003 11:41:23 MONT1.SV0 LIMIT 120.0 115.0 110.0 VOLT [LIN] 105.0 100.0 95.0 90.0 85.0 80.0 1.0 10.0 20.0 30.0 40.0 50.0 60.0 MONTE CARLO [LIN] Major and Minor Distribution In MOS IC processes, manufacturing tolerance parameters have both a major and a minor statistical distribution. ■ The major distribution is the wafer-to-wafer and run-to-run variation. It determines electrical yield. ■ The minor distribution is the transistor-to-transistor process variation. It is responsible for critical second-order effects, such as amplifier offset voltage and flip-flop preference. HSPICE® RF User Guide Z-2007.03 367 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Figure 36 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 RF. 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 368 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Figure 37 Monte Carlo Analysis of RC Time Constant *FILE: NOM1.SP WITH UNIFORM DISTRIBUTION May 15 2003 12:38:49 MONT1.SV0 1 992.750N 900.0N VOLT [LIN] 800.0N 700.0N 600.0N 10 500.0N 9 8 400.0N 7 5 26 3 1 300.0N 0 200.0N 400.0N 600.0N 800.0N 1.0 TIME [LIN] Switched Capacitor Filter Design Capacitors used in switched-capacitor filters consist of parallel connections of a basic cell. Use Monte Carlo techniques in HSPICE RF 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® RF User Guide Z-2007.03 369 Chapter 14: Statistical and Monte Carlo Analysis Monte Carlo Analysis Figure 38 Monte Carlo Distribution cap-to-cap (element) C1a C1b C1a C1b C1c C1d C1c C1d run-to-run (model) You can approach this problem from physical or electrical levels. ■ The physical level relies on physical distributions, such as oxide thickness and polysilicon line width control. ■ The electrical level relies on actual capacitor measurements. Physical Approach: 1. Since oxide thickness control is excellent for small areas on a single wafer, you can use a local variation in polysilicon to control the variation in capacitance for adjacent cells. 2. Next, define a local poly line-width variation and a global (model-level) poly line-width variation. In this example: • The local polysilicon line width control for a line 10 m wide, manufactured with process A, is ±0.02 m for a 1-sigma distribution. • The global (model level) polysilicon line-width control is much wider; use 0.1 m for this example. 3. The global oxide thickness is 200 angstroms with a ±5 angstrom variation at 1 sigma. 4. The cap element is square with local poly variation in both directions. 5. The cap model has two distributions: • poly line-width distribution • oxide thickness distribution. The effective length is: 370 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Leff=Ldrawn - 2 ⋅ DEL The model poly distribution is half the physical per-side values: C1a 1 0 CMOD W=ELPOLY L=ELPOLY C1b 1 0 CMOD W=ELPOLY L=ELPOLY C1C 1 0 CMOD W=ELPOLY L=ELPOLY C1D 1 0 CMOD W=ELPOLY L=ELPOLY $ 10U POLYWIDTH,0.05U=1SIGMA $ CAP MODEL USES 2*MODPOLY .05u= 1 sigma $ 5angstrom oxide thickness AT 1SIGMA .PARAM ELPOLY=AGAUSS(10U,0.02U,1) + MODPOLY=AGAUSS(0,.05U,1) + POLYCAP=AGAUSS(200e-10,5e-10,1) .MODEL CMOD C THICK=POLYCAP DEL=MODPOLY Electrical Approach: The electrical approach assumes no physical interpretation, but requires a local (element) distribution and a global (model) distribution. In this example: ■ You can match the capacitors to ±1% for the 2-sigma population. ■ The process can maintain a ±10% variation from run to run for a 2-sigma distribution. C1a 1 0 CMOD SCALE=ELCAP C1b 1 0 CMOD SCALE=ELCAP C1C 1 0 CMOD SCALE=ELCAP C1D 1 0 CMOD SCALE=ELCAP .PARAM ELCAP=Gauss(1,.01,2) $ 1% at 2 sigma + MODCAP=Gauss(.25p,.1,2) $10% at 2 sigma .MODEL CMOD C CAP=MODCAP Worst Case and Monte Carlo Sweep Example The following example measures the delay and the power consumption of two inverters. Additional inverters buffer the input and load the output. This netlist contains commands for two sets of transient analysis: parameter sweep from -3 to +3-sigma, and a Monte Carlo analysis. It creates one set of output files (mt0 and tr0) for the sigma sweep, and one set (mt1 and tr1) for Monte Carlo. HSPICE® RF User Guide Z-2007.03 371 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example $ inv.sp sweep mosfet -3 sigma to +3 sigma, use measure output .param vref=2.5 sigma=0 .global 1 vcc 1 0 5.0 vin in 0 pwl 0,0 0.2n,5 x1 in 2 inv x2 2 3 inv x3 3 out inv x4 out 4 inv .macro inv in out mn out in 0 0 nch w=10u l=1u mp out in 1 1 pch w=10u l=1u .eom .param mult1=1 + polycd=agauss(0,0.06u,1) xl='polycd-sigma*0.06u' + nactcd=agauss(0,0.3u,1) xwn='nactcd+sigma*0.3u' + pactcd=agauss(0,0.3u,1) xwp='pactcd+sigma*0.3u' + toxcd=agauss(200,10,1) tox='toxcd-sigma*10' + vtoncd=agauss(0,0.05v,1) delvton='vtoncd-sigma*0.05' + vtopcd=agauss(0,0.05v,1) delvtop='vtoncd+sigma*0.05' + rshncd=agauss(50,8,1) rshn='rshncd-sigma*8' + rshpcd=agauss(150,20,1) rshp='rshpcd-sigma*20' * level=28 example model .model nch nmos + level=28 lmlt=mult1 wmlt=mult1 wref=22u lref=4.4u + xl=xl xw=xwn tox=tox delvto=delvton rsh=rshn ... .model pch pmos + level=28 lmlt=mult1 wmlt=mult1 wref=22u lref=4.4u + xl=xl xw=xwp tox=tox delvto=delvtop rsh=rshp + ld=0.08u wd=0.2u acm=2 ldif=0 hdif=2.5u + rs=0 rd=0 rdc=0 rsc=0 rsh=rshp js=3e-04 jsw=9e-10 ... * transient with sweep .tran 20p 1.0n sweep sigma -3 3 .5 .meas s_delay trig v(2) val=vref fall=1 + targ v(out) val=vref fall=1 .meas s_power rms power * transient with Monte Carlo .tran 20p 1.0n sweep monte=100 .meas m_delay trig v(2) val=vref fall=1 + targ v(out) val=vref fall=1 .meas m_power rms power .probe tran v(in) v(1) v(2) v(3) v(4) .end 372 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Transient Sigma Sweep Results The plot in Figure 39 shows the family of transient analysis curves for the transient sweep of the sigma parameter from -3 to +3 from the file inv.tr0. In the sweep, HSPICE RF uses the values of sigma to update the skew parameters, which in turn modify the actual NMOS and PMOS models. Operating-Point Results in Transient Analysis If you want to get OP results after every Monte Carlo simulation in transient analysis, you can add the option opfile to the netlist. OP results will all output to the file *.dp0. Figure 39 Sweep of Skew Parameters from -3 Sigma to +3 Sigma To view the measured results, plot the inv.mt0 output file. The plot in Figure 40 shows the measured pair delay and the total dissipative power, as a function of the parameter sigma. HSPICE® RF User Guide Z-2007.03 373 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Figure 40 Sweep MOS Inverter, Pair Delay and Power: -3 Sigma to 3 Sigma Monte Carlo Results This section describes the output of the Monte Carlo analysis in HSPICE RF. The plot in Figure 41 shows that the relationship between TOX against XL (polysilicon width=transistor length)) is completely random, as set up in the input file. To generate this plot in CosmosScope: 1. Read in the file inv.mt1. 2. Open the Calculator, select TOX (left mouse button), transfer to calculator (middle mouse button), and then select and transfer XL. 3. On the WAVE pulldown in the calculator, select f(x), and then click the plot icon. 4. Using the right mouse button on the plotted waveform, select Attributes to change from the line plot to symbols. 374 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Figure 41 Scatter Plot, XL and TOX The next graph (see Figure 42) is a standard scatter plot showing the measured delay for the inverter pair against the Monte Carlo index number. HSPICE® RF User Guide Z-2007.03 375 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Figure 42 Scatter Plot of Inverter Pair Delay If a particular result looks interesting; for example, if the simulation 68 (monte carlo index=68) produces the smallest delay, then you can obtain the Monte Carlo parameters for that simulation. *** monte carlo index = 68 *** MONTE CARLO PARAMETER DEFINITIONS polycd xl = -1.6245E-07 nactcd xwn = 3.4997E-08 pactcd xwp = 3.6255E-08 toxcd tox = 191.0 vtoncd delvton = -2.2821E-02 delvtop = 4.1776E-02 vtopcd rshncd rshn = 45.16 rshpcd rshp = 166.2 m_delay= 1.7929E-10 targ= 3.4539E-10 m_power= 6.6384E-03 from= 0.0000E+00 trig= to= 1.6610E-10 1.0000E-09 In the preceding listing, the m_delay value of 1.79e-10 seconds is the fastest pair delay. You can also examine the Monte Carlo parameters that produced this result. 376 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example The information on shortest delay and so forth is also available from the statistics section at the end of the output listing. While this information is useful to determine whether the circuit meets specification, it is often desirable to understand the relationship of the parameters to circuit performance. Plotting the results against the Monte Carlo index number does not help for this purpose. You need to generate plots that display a Monte Carlo result as a function of a parameter. For example, Figure 43 shows the inverter pair delay to channel as a function of poly width, which relates directly to device length. Figure 43 Delay as a function of Poly width (XL) Figure 44 shows the pair delay against the TOX parameter. The scatter plot shows no obvious dependence, which means that the effect of TOX is much smaller than XL. To explore this in more detail, set the XL skew parameter to a constant and run a simulation. HSPICE® RF User Guide Z-2007.03 377 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Figure 44 Sensitivity of Delay with TOX The plot in Figure 45 overlays the skew result with the ones from Monte Carlo. The skew simulation traverses the design space with all parameters changing in parallel and then produces a relationship between power and delay, which shows as a single line. Monte Carlo exercises a variety of independent parameter combinations, and shows that there is no simple relationship between the two results. Since the distributions were defined as Gaussian in the netlist, parameter values close to the nominal are more often exercised than the ones far away. With the relatively small number of samples, the chance of hitting a combination at the extremes is very small. In other words, designing for 3-sigma extreme for every parameter is probably not a good solution from the point of view of economy. 378 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Figure 45 Superimposing Sigma Sweep Over Monte Carlo Figure 46 superimposes the required part grades for product sales onto the Monte Carlo plot. This example uses a 250 ps delay and 6.0 mW power dissipation to determine the four binning grades. HSPICE® RF User Guide Z-2007.03 379 Chapter 14: Statistical and Monte Carlo Analysis Worst Case and Monte Carlo Sweep Example Figure 46 Speed/Power Yield Estimation Sorting the results from inv.mt1 yields: ■ Bin1 - 18% ■ Bin2 - 30% ■ Bin3 - 31% ■ Bin4 - 21% If this circuit is representative of the entire chip, then the present yield should be 18% for the premium Bin 1 parts, assuming variations in process parameters as specified in the netlist. Of course this example only shows the principle on how to analyze the Monte Carlo results; there is no market for a device with two of these inverters. 380 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo Simulating the Effects of Global and Local Variations with Monte Carlo Monte Carlo analysis is dependent on a method to describe variability. Four different approaches are available in HSPICE RF: ■ specify distributions on parameters and apply these to instance parameters ■ specify distributions on parameters and apply these to model parameters ■ specify distributions on model parameters using DEV/LOT construct These three methods are still supported in HSPICE RF. In the following sections, the three methods are described. The description relies on test cases, which can be found in the tar file monte_test.tar in directory $<installdir>/demo/hspice/apps. Variations Specified on Geometrical Instance Parameters This method consists of defining parameters with variation using the distribution functions UNIF, AUINF, GAUSS, AGAUSS, and LIMIT. These parameters are then used to generate dependent parameters or in the place of instance parameters. In a Monte Carlo simulation, at the beginning of each sample, new random values are calculated for these parameters. For each reference, a new random value is generated; however, no new value is generated for a derived parameter. Therefore, it is possible to apply independent variations to parameters of different devices, as well as the same variation to parameters of a group of devices. Parameters that describe distributions can be used in expressions, thus it is possible to create combinations of variations (correlations). These concepts are best explained with circuit examples. In the three following examples, variation is defined on the width of a physical resistor, which has a model. If this device was a polysilicon resistor for example, then the variations describe essentially the effects of photoresist exposure and etching on the width of the poly layer. ■ test1.sp has a distribution parameter defined called globw. A parameter called globwidth is assigned the value of globw. The parameter globwidth is assigned a different random value for each Monte Carlo sample. The parameter globwidth is used to define the width of the physical resistors r1, r2, r3, and r4, with model “resistor”. Since parameter globwidth does not have its own distribution defined, but rather gets its value from the parameter globw, the value for globwidth is the same wherever it is used; thus the HSPICE® RF User Guide Z-2007.03 381 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo resistors have the same width for each Monte Carlo sample, and therefore the same resistance. When plotting the simulation results v1, v2, v3, and v4 from the .meas file, the waveforms overlay perfectly. This type of setup is typically used to model global variations, which means variations that affect all devices the same way. ■ test2.sp has a distribution parameter defined called locwidth. This parameter is used to define the width of the physical resistors r1, r2, r3, and r4, with model “resistor”. Since the parameter has its own distribution defined, its value will be different for each reference, and of course for each Monte Carlo sample. Therefore, the resistors will always have different values, and the voltages will be different. This type of setup is typically used to model local variations, which means variations that affect devices in a different way. ■ test3.sp has two kinds of distributions defined: globw/globwidth as in the first example, and locwidth as in the second example. The sum of the two is used to define the width of the resistors. Therefore, the resistors will always have different widths: a common variation due to globwidth and a separate variation due to locwidth. In the example, the distribution for locwidth was chosen as narrower than for globwidth. When overlaying the measurement results, the large common variation can easily be seen; however, all voltages are different. In summary, each reference to a parameter with a specified distribution causes a new random variable to be generated for each Monte Carlo sample. When referencing the parameter on an instance, the effect of a local variation is created. When referencing the parameter on an expression for a second parameter and using the second parameter on an instance, then the effect of a global variation is created. Variations Specified in the Context of Subcircuits The concept explained in the previous section applies also to subcircuits as instances, and instances within subcircuits. Here we again use the example of a physical resistor, with variation of its width. ■ 382 test4.sp uses a subcircuit for each resistor instead of the top-level resistors in test3.sp. On each subcircuit, a parameter “width” is assigned a value by an expression, which is the same for all of them. This value is then passed into the subcircuit and the resistor width gets this value. Because the expression is the same for all subcircuits, the value of parameter “width” will HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo be the same for all subcircuits, thus it expresses a global variation. Therefore all resistors have the same width, and the terminal voltages are the same. ■ In test5.sp, if a different “width” is used for the subcircuits, then the expressions are treated separately, get local variation assigned, and different values are passed into the subcircuit. In test5.sp, the differences inside of the expressions are kept numerically very small, thus the differences from the different values of “locwidth” are dominant and the results look almost identical to the ones from test3.sp. ■ In test6.sp, the resistor width is assigned inside of the subcircuit. The variations get picked up from the top level. Because each subcircuit is a separate entity, the parameter “w” is treated as a separate reference, thus each resistor will have its own value, partly defined through the common value of “globwidth” and partly through the separate value of “locwidth”. ■ test7.sp has two resistors in the subcircuit. Each device in each subcircuit has a separate reference to the variation, therefore each device gets its own value. ■ In test8.sp, the variation definition for “locwidth” has been moved from the top level into the subcircuit. Each resistor has a common global variation and its own local variation. ■ test9.sp assigns the top level variation to a local parameter, which in turn is applied to the width definition of the resistor. This happens independently within each subcircuit, thus we end up with the same values for the resistor pair in each subcircuit, but different values for the different pairs. This technique can be applied to long resistors when a middle terminal is required for connecting capacitance to the substrate. The resulting two resistor pieces will have the same resistance, but it will be different from other resistor pairs. In summary, each subcircuit has its own parameter space, therefore it is possible to put groups of identical components into a subcircuit, and within each group all devices have the same parameter values, but between the groups, parameters are different. When specifying variations on these parameters, the effects of local variations between the groups are created. HSPICE® RF User Guide Z-2007.03 383 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo Variations on a Model Parameter Using a Local Model in Subcircuit If a model is specified within a subcircuit, then the specified parameter values apply only to the devices in the same subcircuit. Therefore, it is possible to calculate the value of a model parameter within the subcircuit; for example, as a function of geometry information. When specifying variations on these parameters, the effects of local variations between subcircuits are created. If this method is used at the extreme with one device per subcircuit, then each device has its own model. This approach leads to a substantial overhead in the simulator and is therefore not recommended. Indirect Variations on a Model Parameter In sections Variations Specified on Geometrical Instance Parameters and Variations Specified in the Context of Subcircuits, variations on geometrical parameters were presented. If we want to specify variations on a model parameter; for example, the threshold of a MOS device, then the approach explained in the previous section with one model per device in a subcircuit could be used. However, this is impractical because the netlist needs to be created to call each device as a subcircuit, and because of the overhead. Since variations are of interest only on a few model parameters, an indirect method of varying model parameters can be used. Some special instance parameters are available for this purpose. For example, for MOS devices, the parameter delvt0 defines a shift in threshold. Referencing a parameter with a distribution as value for delvt0 creates the effect of local threshold variations. A significant number of parameters of this type are available in HSPICE RF for BSIM3 and BSIM4 models. The variations can be tailored for each device depending on its size for example. A disadvantage of this method is that the netlist needs to be parameterized properly to get the correct variations. The process of preparing a basic netlist for Monte Carlo simulations with this approach is tedious and error prone, therefore it is best handled with scripts. Bsim3 supports the following instance parameters: L, w, ad, as, pd, ps, nrd, nrs, rdc, rsc, off, ic, dtemp, delvto, geo, sa, sb, sd, nf, stimod, sa1, sa2, sa3, sa4, sa5, sa6, sa7, sa8, sa9, sa10, sb1, sb2, sb3, sb4, sb5, sb6, sb7, sb8, sb9, sb10, sw1, sw2, sw3, sw4, sw5, sw6, sw7, sw8, sw9, 384 HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo sw10, mulu0, mulua, mulub, tnodeout, rth0, cth0, deltox, delk1, delnfct, and acnqsmod. Bsim4 supports the following instance parameters: L, w, ad, as, pd, ps, nrd, nrs, rdc, rsc, off, ic, dtemp, delvto, geo, rbsb, rbdb, rbpb, rbps, rbpd, trnqsmod, acnqsmod, rbodymod, rgatemod, geomod, rgeomod, nf, min, mulu0, delk1, delnfct, deltox, sa, sb, sd, stimod, sa1, sa2, sa3, sa4, sa5, sa6, sa7, sa8, sa9, sa10, sb1, sb2, sb3, sb4, sb5, sb6, sb7, sb8, sb9, sb10, sw1, sw2, sw3, sw4, sw5, sw6, sw7, sw8, sw9, sw10, xgw, ngcon, sca, scb, scc, sc, delk2, delxj, mulngate, delrsh, delrshg, dellpe0, deldvt0, and mulvsat. (The mulvsat instance parameter is supplied to facilitate efficient modeling of mismatch, local variation, and mechanical stress and proximity effects.) Variations Specified on Model Parameters In this section, we investigate the method of specifying distributions on parameters and using these parameters to define values of model parameters. With this approach, the netlist does not have to be parameterized. The modmonte option can be used to distinguish between global variations (all devices of a particular model have the same parameter set) or local variations (every device has a unique random value for the specified parameters). ■ test10.sp shows a simple case where the model parameter for sheet resistivity is assigned a distribution defined on the parameter rsheet. The results show that all resistors have the same value for each Monte Carlo sample, but a different one for different samples. This setup is useful for studying global variations. ■ test11.sp has .option modmonte=1 added. Now every resistor has a different value. Note that .option modmonte has no effect on any other approach presented here. In summary, assigning parameters with specified distributions to model parameters allows for investigating the effects of global or local variations, but not both. The possibility of selecting one or the other with a simple option is misleading in the sense that the underlying definitions for global and local variations are not the same for a realistic semiconductor technology. HSPICE® RF User Guide Z-2007.03 385 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo Variations Specified Using DEV and LOT The two limitations of the approach described in section Variations Specified on Model Parameters are resolved in this method by specifying global and local variations directly on a model parameter with the syntax: parameterName=parameterValue LOT/distribution LotDist + DEV/distribution DevDist Where, LOT keyword for global distribution DEV keyword for local distribution distribution is as explained in section Variations Specified on Geometrical Instance Parameters LotDist, DevDist characteristic number for the distribution. 3-sigma value for Gaussian distributions. ■ test12.sp has large global and small local variation, similar to the setup in the file test3.sp The result shows four different curves, with a large common part and small separate parts. The amount of variation defined in the two files is the same. The curves look different from the test3.sp results, because different random sequences are used. However the statistical results (sigma) converge for a large number of samples. There is no option available to select only local or only global variations. This can be an obstacle if the file is read-only or encrypted. Combinations of Variation Specifications Specifying distributions on parameters and applying them to model parameters can be used on some models and the DEV/LOT approach on others in the same simulation. 386 ■ test13.sp has DEV/LOT specified for model res1, and the parameter “width” for model res2. The values for the resistors with model res1 are different, and the values for resistors with model res2 are the same. ■ test14.sp is similar to test7.sp and has modmonte=1 specified. All four resistors have different values. However, note that in reality, the sigma for width would be different when simulating local or global variations. ■ test15.sp has instance parameter variations specified on two resistors and DEV/LOT on two others. From the waveforms, v3 and v4 form a first pair, and v1 and v2 a second pair. HSPICE® RF User Guide Z-2007.03 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo It is also possible to mix variations on instance parameters and model parameters in the same setup. ■ test16.sp has small instance parameter variations specified on width and relatively large model parameter variations on the sheet resistivity, rsh. The results show four different waveforms, with a common behavior. ■ test17.sp shows instance and model parameter variations as in the previous test case, but .option modmonte is set to 1, thus the model variations affect every device in a different way. The results show completely independent behavior of all four resistors. If an instance parameter or instance parameter variations and model parameter variations are specified on the same parameter, then the instance parameter always overrides the model parameter. Because only few parameters can be used in both domains, this case is rather seldom, but it needs to be considered to avoid unexpected results. ■ test18.sp has model variation specified on width with a parameter. Two resistors have width also defined on instance. The resistors with instance parameter do not vary at all. The other two resistors vary independently, as expected because .option modmonte is set to 1. ■ test19.sp is similar to test18.sp with .option modmonte set to 0. The two resistors that do not have width defined on the instance line vary together. ■ test20.sp has DEV/LOT specified. Instance parameters override variations on selected resistors. The DEV/LOT approach has no mechanism to describe variation as a function of an element parameter. HSPICE® RF User Guide Z-2007.03 387 Chapter 14: Statistical and Monte Carlo Analysis Simulating the Effects of Global and Local Variations with Monte Carlo 388 HSPICE® RF User Guide Z-2007.03 15 15 Using HSPICE with HSPICE RF Describes how various analysis features differ in HSPICE RF as compared to standard HSPICE. This first section of this chapter describes topics related to transient analysis and the other section describe other differences between HSPICE and HSPICE RF. RF Numerical Integration Algorithm Control 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. You use the SIM_ORDER option to control the amount of Backward-Euler (BE) to mix with the Trapezoidal (TRAP) method for hybrid integration. For example, .OPTION SIM_ORDER=x Setting SIM_ORDER to its lowest value selects Backward-Euler integration algorithm, and setting it to its highest value selects Trapezoidal integration. For the syntax and description of this control option, see .OPTION SIM_ORDER in the HSPICE and HSPICE RF Command Reference. RF Transient Analysis Accuracy Control The default time step method in HSPICE RF mixes timestep algorithms Trapezoidal and second-order Gear (Gear-2). This yields a more accurate scheme than Trapezoidal or Backward-Euler. Also, detection of numerical HSPICE® RF User Guide Z-2007.03 389 Chapter 15: Using HSPICE with HSPICE RF RF Transient Analysis Accuracy Control oscillations inserts fewer Backward-Euler steps than in previous HSPICE versions. .OPTION SIM_ACCURACY You use the SIM_ACCURACY option to modify the size of timesteps in HSPICE RF. For example, .OPTION SIM_ACCURACY=<value> 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. You can apply different accuracy settings to different blocks or time intervals. The syntax to set accuracy on a block, instance, or time interval is similar to the settings used for a power supply. Note: An .OPTION SIM_ACCURACY takes precedence over an.OPTION ACCURATE. For the syntax and description of this control option, see .OPTION SIM_ACCURACY in the HSPICE and HSPICE RF Command Reference. Algorithm Control In HSPICE RF, you can select the Backward-Euler, Trapezoidal, Gear, or hybrid method algorithms. Each of these algorithms has its own advantages and disadvantages for specific circuit types. These methods have tradeoffs related to accuracy, avoidance of numerical oscillations, and numerical damping of circuit oscillations. For pre-charging simulation or timing critical simulations, the Trapezoidal algorithm usually improves accuracy. .OPTION METHOD You use the METHOD option to select a numeric integration method for a transient analysis. HSPICE RF supports three basic timestep algorithms: Trapezoidal (TRAP), second-order Gear (Gear-2), and Backward-Euler (BE). Backward-Euler is the 390 HSPICE® RF User Guide Z-2007.03 Chapter 15: Using HSPICE with HSPICE RF RF Transient Analysis Accuracy Control same as first-order Gear. Also, HSPICE RF supports a hybrid algorithm (TRAPGEAR), 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. The TRAPGEAR 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. For the syntax and description of this control option, see .OPTION METHOD in the HSPICE and HSPICE RF Command Reference. .OPTION MAXORD You use the MAXORD option to select the maximum order of integration for the GEAR method. Either the first-order Gear (Backward-Euler), or the secondorder Gear (Gear-2) integration method. For the syntax and description of this control option, see .OPTION MAXORD in the HSPICE and HSPICE RF Command Reference. .OPTION SIM_ORDER You use the SIM_ORDER option to control the amount of Backward-Euler (BE) to mix with the Trapezoidal method for hybrid integration. This option affects time stepping when you set .OPTION METHOD to TRAP or TRAPGEAR. For the syntax and description of this control option, see .OPTION SIM_ORDER in the HSPICE and HSPICE RF Command Reference. .OPTION SIM_TG_THETA You use the SIM_TG_THETA option to control the amount of Gear-2 method to mix with trapezoidal integration for the hybrid TRAPGEAR method. For the syntax and description of this control option, see .OPTION SIM_TG_THETA in the HSPICE and HSPICE RF Command Reference. .OPTION SIM_TRAP You use the SIM_TRAP option to change the default SIM_TG_THETA to 0, so that method=trapgear acts like METHOD=TRAP. HSPICE® RF User Guide Z-2007.03 391 Chapter 15: Using HSPICE with HSPICE RF RF Transient Analysis Output File Formats For the syntax and description of this control option, see .OPTION SIM_TRAP in the HSPICE and HSPICE RF Command Reference. .OPTION PURETP You use the PURETP option to turn off insertion of Backward-Euler (BE) steps due to auto-detection of numerical oscillations. For the syntax and description of this control option, see .OPTION PURETP in the HSPICE and HSPICE RF Command Reference. .OPTION SIM_OSC_DETECT_TOL You use the SIM_OSC_DETECT_TOL option to specify the tolerance for detecting numerical oscillations. If HSPICE RF detects numerical oscillations, it inserts Backward-Euler (BE) steps. Smaller values of this tolerance result in fewer BE steps. For the syntax and description of this control option, see .OPTION SIM_OSC_DETECT_TOL in the HSPICE and RF Command Reference. RF Transient Analysis Output File Formats The default output format for transient analysis in HSPICE RF is the same as in HSPICE: the .tr0 file format. See Transient Analysis in the HSPICE Simulation and Analysis User Guide. HSPICE RF supports these output formats, which are described in this section: ■ Tabulated Data Output ■ WDB Output Format ■ XP Output Format ■ NW Output Format ■ VCD Output Format ■ turboWave Output Format (tw) ■ Undertow Output Format (ut) ■ CSDF Output Format If your netlist includes an unsupported output format, HSPICE RF prints a warning message, indicating that the selected format is unsupported. HSPICE RF then automatically defaults the output to TR0 format. 392 HSPICE® RF User Guide Z-2007.03 Chapter 15: Using HSPICE with HSPICE RF RF Transient Analysis Output File Formats You can use the waveform viewer to view certain output formats: ■ wdb: XP/CosmosScope (Recommended) ■ nw: XP/AvanWaves ■ xp: XP/AvanWaves/CosmosScope Note: If your waveform file is larger than 2GB, use split waveforms. Tabulated Data Output HSPICE RF outputs all analog waveforms specified in a .PRINT statement. HSPICE RF saves these waveforms as ASCII tabulated data, into a file with the .PRINT extension. To display waveforms graphically, CosmosScope can directly read the tabulated data. For more information about CosmosScope, see the CosmosScope User’s Guide and Reference. Note: Tabulated data excludes waveforms specified in .PROBE statements. WDB Output Format You can use the waveform database (WDB) output format in .OPTION POST. It was developed for maximum efficiency. The output file is *.wdb#. For example, to output to a *.wdb# file, enter: .OPTION POST=wdba 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 CosmosScope extracts one signal at a time. This means that CosmosScope does not need to read the entire output file to display a single waveform. 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. HSPICE® RF User Guide Z-2007.03 393 Chapter 15: Using HSPICE with HSPICE RF RF Transient Analysis Output File Formats Furthermore, the WDB format is usually more compact than XP and NW (described later in this section). However, if the NW file is already very small, then WDB offers little advantage in size or speed. You can compress WDB files. For additional information, see Compressing Analog Files on page 396. TR Output Format HSPICE RF stores simulation results for analysis by using the AvanWaves graphical interface method. For example, these commands output a *.tr# file in TR format: ■ .OPTION POST=1 saves the results in binary format ■ .OPTION POST=2 saves the results in ASCII format. XP Output Format HSPICE RF outputs XP binary format to a file with the .xp# extension. This format is compatible with the HSPICE TR binary format. For example, to output to a *.xp# file, enter: .OPTION POST=xp NW Output Format HSPICE RF outputs the NW format to a file with the .nw# extension. Synopsys developed this format; you need a Synopsys waveform display tool to process a file in NW format. For example, to output to a *.nw# file, enter: .OPTION POST=nw You can compress NW files. For additional information, see Compressing Analog Files on page 396. VCD Output Format To output your waveforms from HSPICE RF in VCD (Value Change Dump) format, set the VCD option in conjunction with the .LPRINT statement. For example, 394 HSPICE® RF User Guide Z-2007.03 Chapter 15: Using HSPICE with HSPICE RF RF Transient Analysis Output File Formats .OPTION VCD .LPRINT (0.5 4.5) v(0) v(2) v(6) .LPRINT Statement You use the .LPRINT statement to produce output in VCD file format from transient analysis. For example, .LPRINT (v1,v2) output_varable_list For additional information, see .LPRINT in the HSPICE and HSPICE RF Command Reference. turboWave Output Format To use turboWave output format TW, enter: .OPTION POST=tw This format supports analog compression as described in Compressing Analog Files on page 396. Undertow Output Format To use Veritools Undertow output format UT, enter: .OPTION POST=ut This format supports analog compression as described in Compressing Analog Files on page 396. The waveform list in UT format now displays in a hierarchical structure, rather than one flat level as in previous versions. CSDF Output Format To use CSDF output format CSDF, enter: .OPTION POST=csdf .OPTION csdf [overrides .OPTION POST setting] HSPICE® RF User Guide Z-2007.03 395 Chapter 15: Using HSPICE with HSPICE RF Compressing Analog Files Compressing Analog Files Analog compression eliminates unnecessary data points from a HSPICE RF voltage or current waveform to reduce the size of the waveform file. Eliminating Voltage Datapoints You use the SIM_DELTAV option to determine the selection criteria for HSPICE RF voltage waveforms in WDB or NW format. For example, .OPTION 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. Figure 47 Analog Compression Formats NW and WDB both eliminate these data points, which are within DELTAV or DELTAI of the previous data point, and are not ON the plotted waveform line. NW retains these data points that are ON the line, plotting 3 segments. But WDB eliminates these data points, plotting only ONE segment for this line. For a additional information, see .OPTION SIM_DELTAV in the HSPICE and HSPICE RF Command Reference. Eliminating Current Datapoints You use the SIM_DELTAI option to determine the selection criteria for HSPICE RF current waveforms in WDB or NW format. For example, 396 HSPICE® RF User Guide Z-2007.03 Chapter 15: Using HSPICE with HSPICE RF Compressing Analog Files .OPTION SIM_DELTAI=<value> For a additional information, see .OPTION SIM_DELTAI in the HSPICE and RF Command Reference. HSPICE® RF User Guide Z-2007.03 397 Chapter 15: Using HSPICE with HSPICE RF Compressing Analog Files 398 HSPICE® RF User Guide Z-2007.03 16 16 Advanced Features Describes how to invoke HSPICE RF and how to perform advanced tasks, including redirecting input and output. HSPICE RF accepts a netlist file from stdin and delivers the ASCII text simulation results to an HTML file or to stdout. Error and warning messages are forwarded to standard error output. This chapter describes how to do this as well as how to invoke HSPICE RF and redirect input and output. Creating a Configuration File You can create a configuration file, called .hspicerf, to customize your HSPICE RF simulation. HSPICE RF first searches for .hspicerf in your current working directory, then in your home directory as defined by $HOME. The configuration options listed in Table 29 are available for your use. HSPICE® RF User Guide Z-2007.03 399 Chapter 16: Advanced Features Creating a Configuration File Table 29 Configuration File Options Keyword Description Example flush_waveform Flushes a waveform. If you do not specify a percentage, then the default value is 20%. flush_waveform percent% ground_floating_ node Uses .IC statements to set floating nodes in a ground_floating_ circuit to ground. You can select three options for node 1 grounding floating nodes: ■ ■ ■ If set to 1, grounds only floating nodes (gates, bulk, control nodes, non-rail bulk) that are included in the .IC set. If set to 2, adds unconnected terminals to this set. If set to 3, uses .IC statements to ground all floating nodes, including dangling terminals. hier_delimiter Changes the delimiter for subcircuit hierarchies hier_delimiter / from “.” to the specified symbol. html Stores all HSPICE RF output in HTML format. htmlhspicerf test This example creates a file named test.html in the current directory. integer_node Removes leading zeros from node names. For example, HSPICE RF considers 0002 and 2 to be the same node. integer_node Without this keyword, 0002 and 2 are two separate nodes. max_waveform_size Automatically limits the waveform file size. ■ ■ ■ 400 max_waveform_ If the number is less than 5000, HSPICE RF size 2000000000 resets it to 2G. If you do not set the number, HSPICE RF uses the default, 2G. If you do not set the line, the file size has no limit. HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Creating a Configuration File Table 29 Configuration File Options (Continued) Keyword Description Example negative_td Allows negative time delay input in pwl (piecewise linear with repeat), pl (piecewise linear), exp (exponential, rising time delay only), sin (damped sinusoidal), pulse (trapezoidal pulse), and am (amplitude modulation) formats. If you do not set negative_td, a negative time delay defaults to zero. port_element_ voltage_ matchload Allows the alternate Port element definition. A Port element consists of a voltage source in series with a resistor. port_element_ voltage_ matchload For the explanation that follows, let the userspecified DC, AC, or transient value of the Port element be V, and let the voltage across the overall port element be Vp. By default, HSPICE RF will set the internal voltage source value to V. The value of Vp will be lower than V, depending on the internal impedance and the network's input impedance. With the alternate definition, the internal voltage source value is adjusted to 2*V, so that Vp=V when the Port element's impedance is matched with the network input impedance. The actual value of Vp will still depend on the port and network impedances. rcxt_divider Defines the hierarchy delimiter in the active nodes file in RCXT format. skip_nrd_nrs Directs HSPICE RF to consider transistors with skip_nrd_nrs matching geometries (except for NRD and NRS) as identical for pre-characterization purposes. unit_atto Activates detection of the “atto.” unit. Otherwise, unit_atto HSPICE RF assumes that “a” represents “amperes.” v_supply Changes the default voltage supply range for characterization. v_supply 3 wildcard_left_range Begins range expression. wildcard_left_ range [ HSPICE® RF User Guide Z-2007.03 rcxt_divider / 401 Chapter 16: Advanced Features Using Wildcards in HSPICE RF Table 29 Configuration File Options (Continued) Keyword Description Example wildcard_match_all Matches any group of characters. wildcard_match_ all * wildcard_match_one Matches any single character. wildcard_match_ one ? wildcard_right_range Ends range expression. wildcard_right_ range ] Note: For more information about wildcards, see Using Wildcards in HSPICE RF on page 402. Inserting Comments in a .hspice File To insert comments into your .hspicerf file, include a number sign character (#) as the first character in a line. For example, this configuration file shows how to use comments in a .hspicerf file: # sample configuration file # the next line of code changes the delimiter # for subcircuit hierarchies from "," to "^" hier_delimiter ^ # the next line of code matches any groups of "*" characters wildcard_match_all * # the next line of code matches one "?" character wildcard_match_one ? # the next line of code begins the range expression with # the "[" character wildcard_left_range [ # the next line of code ends the range expression with # the "]" character wildcard_right_range ] Using Wildcards in HSPICE RF You can use wildcards to match node names. HSPICE RF uses wildcards somewhat differently than standard HSPICE. 402 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Limiting Output Data Size Before using wildcards, you must define the wildcard configuration in a .hspicerf file. For example, you can define the following wildcards in a .hspicerf file: file .hspicerf wildcard_match_one wildcard_match_all wildcard_left_range wildcard_right_range ? * [ ] The .PRINT, .PROBE, .LPRINT, and .CHECK statements support wildcards in HSPICE RF. For more information about using wildcards in an HSPICE configuration file, see Using Wildcards in PRINT and PROBE Statements in the HSPICE Simulation and Analysis User Guide. Limiting Output Data Size 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 reduce 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 SIM_POSTTOP Option You use the SIM_POSTTOP option to limit the data written to your waveform file to data from only the top n level nodes. This option outputs instances up to n levels deep. For example, HSPICE® RF User Guide Z-2007.03 403 Chapter 16: Advanced Features Limiting Output Data Size .OPTION SIM_POSTTOP=<n> Note: To enable the waveform display interface, you also need the POST option. For additional information, see .OPTION SIM_POSTTOP in the HSPICE and HSPICE RF Command Reference. SIM_POSTSKIP Option You use the SIM_POSTSKIP to have the SIM_POSTTOP option skip any instances and their children that the subckt_definition defines. For example, .OPTION SIM_POSTSKIP=<subckt_definition> For additional information, see .OPTION SIM_POSTSKIP in the HSPICE and HSPICE RF Command Reference. SIM_POSTAT Option You use the SIM_POSTAT option to limit the waveform output to only the nodes in the specified subcircuit instance. For example, .OPTION SIM_POSTAT=<instance> This option can be used in conjunction with the SIM_POSTTOP option and when present, has precedence over the SIM_POSTSKIP option. For additional information, see .OPTION SIM_POSTAT in the HSPICE and HSPICE RF Command Reference. SIM_POSTDOWN Option You use the SIM_POSTDOWN option to include an instance and all children of that instance in the output. For example, .OPTION SIM_POSTDOWN=<instance> It can be used in conjunction with the SIM_POSTTOP option and when present, has precedence over the SIM_POSTSKIP option. 404 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Probing Subcircuit Currents For additional information, see .OPTION SIM_POSTDOWN in the HSPICE and HSPICE RF Command Reference. SIM_POSTSCOPE Option You use the SIM_POSTSCOPE option to specify the signal types to probe from within a scope. For example, .OPTION SIM_POSTSCOPE=net|port|all For additional information, see .OPTION SIM_POSTSCOPE in the HSPICE and HSPICE RF Command Reference. Probing Subcircuit Currents To provide subcircuit power probing utilities, HSPICE RF uses the X() and X0() extended output variables. You can use these X variables in .PROBE, .PRINT, or .MEASURE statements. The following syntax is for the output variable X(): X (subcircuit_node_path) X0 (subcircuit_node_path) subcircuit_node_path specifies the subcircuit path and the subcircuit node name definition. The node must be either an external node in a subcircuit definition or a global node. X() returns the total current flowing into a subcircuit branch, including all lower subcircuit hierarchies. X0() returns only current flowing into a subcircuit branch, minus any current flowing into lower subcircuit hierarchies. Figure 48 on page 406 illustrates the difference between the X() and X0 () variables. The dotted line boxes represent subcircuits, and the black circles are the external nodes. The X(X1.vc1) path returns the current of the X1subcircuit, through the vc1 node, including the current to the X1.X1 and X1.X2 subcircuits as represented by the white (black outlined) arrows. In contrast, X0(X1.vc2) returns only the current flowing through vc2 to the top level of the X1 subcircuit as shown by the black arrows. HSPICE® RF User Guide Z-2007.03 405 Chapter 16: Advanced Features Probing Subcircuit Currents Figure 48 Probing Subcircuit Currents VDD1 VDD2 X0(X1.vc2) X(X1.vc1) vc1 X(X2.vd2) vc2 X1 vd1 vd2 X2 X1.X1 X1.X2 Example 1 In this example, the first five lines constitute the definition of the sb1 subcircuit with external nodes named node1, node2, and clr. The line beginning with X1 is an instance of sb1 with nodes named; ■ 11 (references node1) ■ 12 (references node2) ■ 0 (references clr) .subckt sb1 node1 node2 clr * subckt elements R1 node1 node2 1K C1 clr node1 1U .ends * subcircuit instance X1 11 12 0 sb1 .PRINT X(X1.node1) ‘X(X1.clr) + I(X1.R1)’ To find the current flowing into node 11 of the X1 subcircuit instance, this example uses the X() variable. HSPICE RF maps node 11 to the node1 external node as shown in the first part of the .PRINT statement. The latter half of the .PRINT statement illustrates that you can combine the X() variable with I() variables. 406 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Generating Measurement Output Files Example 2 In this example, the X() variable finds the current through the in node of the S1 subcircuit. .subckt S1 in out R1 in inp 1K C1 inp 0 1u R2 in out 1K .PROBE X(in) .ends Generating Measurement Output Files You can make all of the same measurements with the .MEASURE statement in HSPICE RF as you can in HSPICE. The results of the .MEASURE statements appear in a file with one of the following filename extensions: ■ .mt# for measurements in transient analysis ■ .ms# for measurements in DC analysis ■ .ma# for measurements in AC analysis ■ .mb# for measurements in HB analysis ■ .mp# for measurements in HBNOISE analysis For more information about .MEASURE statements, see the HSPICE and HSPICE RF Command Reference. Optimization Like HSPICE, HSPICE RF employs an incremental optimization technique. This technique solves the DC parameters first, then the AC parameters, and finally the transient parameters. To perform optimization, create an input netlist file that specifies: ■ Optimization parameters with upper and lower boundary values along with an initial guess. ■ An AC, DC, TRAN, HB, or HBOSC optimization statement. HSPICE® RF User Guide Z-2007.03 407 Chapter 16: Advanced Features Optimization ■ An optimization model statement. ■ Optimization measurement statements for optimization parameters. If you provide the input netlist file, optimization specifications, limits, and initial guess, then the optimizer reiterates the simulation until it finds an optimized solution. Usage Notes and Examples ■ Optimization works for TRAN, AC, DC, HB, HBOSC, and HBAC analyses. ■ You can add the GOAL options in every meaningful .MEASURE statement, like FIND-WHEN, FIND-AT, and so forth. ■ A data sweep is not required to be defined in the .HB statement for HB optimization to use the measured result from .MEASURE HBNOISE, PHASENOISE, or HBTRAN statements. Therefore, parameter sweep is not supported for this type of optimization. ■ Optimize multiple parameters with multiple goals by selecting .MODEL OPT LEVEL=0 (modified Lavenberg-Marquardt method). ■ Optimize single parameters in single measurement situations by selecting .MODEL OPT LEVEL=1 (bisection method). ■ Examples • Setting optimization parameters .param W=opt1(231u, 100u, 800u) .param Rs=opt1(10,8,20) • Optimization analysis statement .HB tones=2.25g 2.5g nharms=6,3 + sweep Pin:dbm -30 0 2 + sweep optimize = opt1 + results = gain $measure result to tune the parameters + model= optmod1 • Selecting an optimization model .model optmod1 opt level=1 $Bisection method + itropt=40 relin=1e-4 relout=1e-6 $ accuracy settings • Measurement statements to tune the optimization parameters .measure HB vif find vdb(if+)[-1,1] at 10e-6 .measure HB vrf find vdb(rf+)[0,1] at 10e-6 .measure HB gain=param('vif-vrf') goal=-2 408 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Optimization • Measurement statement to find the fundamental frequency from HB analysis .measure HB frequency_max FIND ‘HERTZ[1]’ at=0 Optimizing AC, DC. and TRAN Analyses The HSPICE syntax is followed for optimizing AC, DC. and TRAN analyses. The required statements are: ■ Optimization .PARAM statement .PARAM <ParamName>=OPTxxx(<Init>,<LoLim>,<HiLim>) ■ Optimizing .TRAN statement .TRAN tincr1 tstop1 <tincr2 tstop2 ... tincrN tstopN> + SWEEP OPTIMIZE=OPTxxx RESTULTS=measname MODEL=optmod ■ Optimizing .MODEL statement .MODEL mname OPT LEVEL=[0|1] Where: • 0 specifies the Modified Levenberg-Marquardt method. You would use this setting with multiple optimization parameters and goals. • 1 specifies the Bisection method. You would use this setting with one optimization parameter. Optimizing HB Analysis There are two types of optimizations with HB analyses: ■ Optimization with only HB measurements ■ Optimization with HBNOISE, PHASENOISE, or HBTRAN measurements Optimization With HB Measurements The required statements are: HSPICE® RF User Guide Z-2007.03 409 Chapter 16: Advanced Features Optimization ■ Analysis statement .HB TONES=<f1>[<f2> ... <fn>] <NHARMS=<h1>,<h2> ... <hn>> + SWEEP parameter_sweep OPTIMIZE=OPTxxx RESULT=measname + MODEL=mname ■ Measure statement .MEASURE HB measname FIND out_var1 AT=val GOAL=val Optimization With HBNOISE, PHASENOISE, or HBTRAN Measurements The required statements are: ■ Analysis statement .HB TONES=<f1>[<f2> ... <fn>] <NHARMS=<h1>,<h2> ... <hn>> + SWEEP OPTIMIZE=OPTxxx RESULT=measname MODEL=mname For example, .HBOSC tones=1g nharms = 5 optimize = opt1 + result = y1, y2 model = m1 .model m1 opt level=0 .PHASENOISE dec 1 1k 1g .meas phasenoise y1 find phnoise at 10k goal = -150dbc .meas phasenoise y2 RMSJITTER phnoise units = sec goal = 1.0e-12 ■ Measure statement .MEASURE HBNOISE measname FIND out_var1 AT=val GOAL=val .MEASURE PHASENOISE measname FIND out_var1 AT=val + GOAL=val .MEASURE HBTRAN measname FIND out_var1 AT=val GOAL=val Optimizing HBOSC Analysis There are two types of optimizations with .HBOSC analyses: ■ Optimization with only HB measurements ■ Optimization with HBNOISE, PHASENOISE, or HBTRAN measurements Optimization With HB Measurements The required statements are: 410 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Using CHECK Statements ■ Analysis statement .HBOSC TONES=<f1>[<f2> ... <fn>] <NHARMS=<h1>,<h2> ... <hn>> + SWEEP parameter_sweep OPTIMIZE=OPTxxx RESULT=measname + MODEL=mname ■ Measure statement .MEASURE HB measname FIND out_var1 AT=val GOAL=val Optimization With HBNOISE, PHASENOISE, or HBTRAN Measurements The required statements are: ■ Analysis statement .HBOSC TONES=<f1>[<f2> ... <fn>] <NHARMS=<h1>,<h2> ... <hn>> + SWEEP OPTIMIZE=OPTxxx RESULT=measname MODEL=mname For example, .HBOSC tones=1g nharms = 5 sweep x 1 5 1 optimize = opt1 + result = y1, y2 model = m1 .model m1 opt level=0 .PHASENOISE dec 1 1k 1g .meas phasenoise y1 find phnoise at 10k goal = -150dbc .meas phasenoise y2 RMSJITTER phnoise units = sec goal = 1.0e-12 Measure statement— .MEASURE HBNOISE measname FIND out_var1 AT=val GOAL=val .MEASURE PHASENOISE measname FIND out_var1 AT=val + GOAL=val .MEASURE HBTRAN measname FIND out_var1 AT=val GOAL=val Optimization with HBNOISE, PHASENOISE or HBTRAN measurements must not be used in combination with HB measurement optimization as shown in Optimization With HB Measurements. Using 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 HSPICE® RF User Guide Z-2007.03 411 Chapter 16: Advanced Features Using CHECK Statements ■ Setup and Hold Verification ■ IR Drop Detection The results of these statements appear in a file with an .err extension. To prevent creating unwieldy files, HSPICE RF reports only the first 10 violations for a particular check in the .err file. Setting Global Hi/Lo Levels You use the .CHECK GLOBAL_LEVEL statement to globally set the desired high and low definitions for all CHECK statements. For example, .CHECK GLOBAL_LEVEL (hi lo hi_th lo_th) Values for hi, lo, and the thresholds are defined by using this statement. For syntax and description of this statement, see .CHECK GLOBAL_LEVEL in the HSPICE and HSPICE RF Command Reference. Slew, Rise, and Fall Conditions You use the .CHECK SLEW statement to verify that a slew rate occurs within the specified window of time. For example, .CHECK SLEW (min max) node1 <node2 ...> <(hi lo hi_th lo_th) Figure 49 SLEW Example 3.3 2.6 0.7 0.0 1ns < t < 3ns For syntax and description of this statement, see .CHECK SLEW in the HSPICE and HSPICE RF Command Reference. You use the .CHECK RISE statement to verify that a rise time occurs within the specified window of time. For example, 412 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Using CHECK Statements .CHECK RISE (min max) node1 <node2 ...> <(hi lo hi_th lo_th)> Figure 50 RISE Time Example HI HI_thresh LO_thresh LO 1.5 ns < t < 2.2 ns For syntax and description of this statement, see .CHECK RISE in the HSPICE and HSPICE RF Command Reference. You use the .CHECK FALL statement to verify that a fall time occurs within the specified window of time. For example, .CHECK FALL (min max) node1 <node2 ...> <(hi lo hi_th lo_th)> For syntax and description of this statement, see .CHECK FALL in the HSPICE and HSPICE RF Command Reference. Edge Timing Verification The edge condition verifies that a triggering event provokes an appropriate RISE or FALL action, within the specified time window. You use the .CHECK EDGE statement to verify this condition. For example, .CHECK EDGE (ref RISE|FALL min max RISE|FALL) + node1 < node2 . . . > < (hi lo hi_th low_th) > Figure 51 EDGE Example voutA CLK HI HI_thresh LO_thresh LO 1ns < t < 3 ns HSPICE® RF User Guide Z-2007.03 413 Chapter 16: Advanced Features Using CHECK Statements For syntax and description of this statement, see .CHECK EDGE in the HSPICE and HSPICE RF Command Reference. Setup and Hold Verification You use the .CHECK SETUP and .CHECK HOLD statements to ensure that specified signals do not switch for a specified period of time. For example, .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) > ■ For a SETUP condition, this is the minimum time before the triggering event, during which the specified nodes cannot rise or fall. Figure 52 SETUP Example nodeA v1 HI HI_thresh LO_thresh LO t >=2ns For syntax and description of this statement, see .CHECK SETUP in the HSPICE and HSPICE RF Command Reference. ■ 414 For a HOLD condition, this is minimum time required after the triggering event, before the specified nodes can rise or fall. HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features POWER DC Analysis Figure 53 HOLD Example vin* nodeA HI HI_thresh LO_thresh LO t >=2ns For syntax and description of this statement, see .CHECK HOLD in the HSPICE and HSPICE RF Command Reference. IR Drop Detection You use the .CHECK IRDROP statement to verify that the IR drop does not exceed, or does not fall below, a specified value for a specified duration. For example, .CHECK IRDROP ( volt_val time ) node1 < node2 . . . > + < ( hi lo hi_th low_th ) > Figure 54 IR Drop Example v1 -2 volts t <=1ns For syntax and description of this statement, see .CHECK IRDROP in the HSPICE and HSPICE RF Command Reference. POWER DC Analysis You use the .POWERDC (standby current) statement to calculate the DC leakage current of a design hierarchy. For example, .POWERDC <keyword> <subckt_name1...> HSPICE® RF User Guide Z-2007.03 415 Chapter 16: Advanced Features POWER DC Analysis This statement 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 lists the sum of the power of each port in the subcircuit. You use the SIM_POWERDC_HSPICE option to increase the accuracy of operating point (OP) calculations. Or for even higher accuracy in operating point calculations, you use the SIM_POWERDC_ACCURACY option. For syntax and description of this statement and options, see .POWERDC, .OPTION SIM_POWERDC_ACCURACY or .OPTION SIM_POWERDC_HSPICE in the HSPICE and HSPICE RF Command Reference. Power DC Analysis 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) 416 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features POWER Analysis *** 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 ....... Min(A) Avg(A) Min(A) Avg(A) POWER Analysis The .POWER statement in HSPICE RF creates a table, which by default contains the measurements for AVG, RMS, MAX, and MIN for every signal specified. For example, .POWER <signals> <REF=vname FROM=start_time TO=end_time> By default, the scope of these measurements are set from 0 to the maximum timepoint specified in the .TRAN statement. For syntax and description of .POWER statement, see ..POWER in the HSPICE and HSPICE RF Command Reference. Example 1 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). .power x1.in .tran 4ps 100ps Example 2 You can use the FROM and TO times to specify a separate measurement start and stop time for each signal. In this example: HSPICE® RF User Guide Z-2007.03 417 Chapter 16: Advanced Features Detecting and Reporting Surge Currents ■ The scope for simulating the x2.in signal is from 20ps to 80ps. ■ The scope for simulating the x0.in signal is from 30ps to 70ps. .param myendtime=80ps .power x2.in REF=a123 from=20ps to=80ps .power x0.in REF=abc from=30ps to=’myendtime - 10ps’ Setting Default Start and Stop Times In addition to using FROM and TO times in a .POWER statement, you can also use the SIM_POWERSTART and SIM_POWERSTOP options with .POWER statements to specify default start and stop times for measuring signals during simulation. These times apply to all signals that do not have their own defined FROM and TO measurement times. For example, .OPTION SIM_POWERSTART=<time> .OPTION SIM_POWERSTOP=<time> These options control the power measurement scope; the default is for the entire run. For syntax and description of these options, see .OPTION SIM_POWERSTART or .OPTION SIM_POWERSTOP in the HSPICE and HSPICE RF Command Reference. Controlling Power Analysis Waveform Dumps You use the SIM_POWERPOST option to control power analysis waveform dumping. For example, .OPTION SIM_POWERPOST=ON|OFF Considering the potentially enormous number of signals, there is no waveform dumping by default for the signals in the .POWER statement. Setting SIM_POWERPOST=ON turns on power analysis waveform dumping. Detecting and Reporting Surge Currents The .SURGE statement in HSPICE RF automatically detects and reports a current surge that exceeds the specified surge tolerance. For example, 418 HSPICE® RF User Guide Z-2007.03 Chapter 16: Advanced Features Detecting and Reporting Surge Currents .SURGE surge_threshold surge_width node1 < node2 .... noden > This statement reports any current surge that is greater than surge_threshold for a duration of more than surge_width. For additional information, see .SURGE in the HSPICE and RF Command Reference. HSPICE® RF User Guide Z-2007.03 419 Chapter 16: Advanced Features Detecting and Reporting Surge Currents 420 HSPICE® RF User Guide Z-2007.03 Index Symbols !GND node 79 A abs(x) function 101 absolute power function 101 value function 101 .AC statement 353 accuracy control 389 acos(x) function 100 adding library data 85 AGAUSS keyword 363 algebraic expressions 99 algorithm linear acceleration 346 nonlinear perturbation 242 numerical integration 389, 390 periodic AC 242 .ALTER blocks 82–83, 84 statement 83, 84, 85 amplifier 15, 19 amplifier, IP3 22 analysis data driven 350, 351 Monte Carlo 351, 359, 359–380 oscillator 229 phase noise 238 statistical 354–380 Taguchi 350 temperature 350, 352 time domain steady-state 219 worst case 350, 354–380 yield 350 arccos(x) function 100 arcsin(x) function 100 arctan(x) function 101 arithmetic operators 100 ASIC libraries 92 asin(x) function 100 atan(x) function 101 AUNIF keyword 363 average deviation 351 B B# node name in CSOS 80 backslash continuation character 100 Backward-Euler algorithm 389, 390 integration 389, 390 Behavioral resistors 118 BJTs elements, names 162 block elements 138 broadband phasenoise 243 broadband phasenoise algorithm 243 buffer 155 C C Element (capacitor) 123 capacitance manufacturing variations 369 capacitor charge-based 122 element 119, 123 frequency-dependent 124 linear 123 cell characterization 350 charge-based capacitor 122 .CHECK EDGE statement 413 .CHECK FALL statement 413 .CHECK GLOBAL_LEVEL statement 412 .CHECK HOLD statement 414 .CHECK IRDROP statement 415 .CHECK RISE statement 412 .CHECK SETUP statement 414 .CHECK SLEW statement 412 421 Index D choke elements 138 circuit description syntax 9 circuits description syntax 70 reusable 87 subcircuit numbers 79 temperature 353 See also subcircuits clock source, random jitter 191 CMOS GPS VCO 31 Colpitts oscillator 28 .command .PRINT ENV 315 command .PROBE ENV 315 commands hspicerf 9 PTDNOISE 281 comment line netlist 71 comparing results 41 compression of input files 57 config file hspicerf 399 configuration file 399 example 402 configuration options flush_waveform 400 ground_floating_ node 400 hier_delimiter 400 html 400 integer_node 400 max_waveform_size 400 negative_td 401 port_element_ voltage_ matchload 401 rcxt_divider 401 unit_atto 401 v_supply 401 wildcard_left_range 401 wildcard_match_all 402 wildcard_match_one 402 wildcard_right_range 402 continuation character, parameter strings 100 continuation of line netlist 72 cos(x) function 100 cosh(x) function 101 Cosmos-Scope 12 422 coupled inductor element 134 D .DATA statement 81 data-driven analysis 81, 350, 351 db(x) function 101 DC block elements 138 .DC statement 353 DDL 91 DDLPATH environment variable 91 decibel function 101 DEFW option 108 .DEL LIB statement 68 in .ALTER blocks 83, 84 with .ALTER 85 with .LIB 85 with multiple .ALTER statements 84, 85 DELVTO model parameter 355 demo files 55 55 demonstration files, RF 55 demonstration input files 55 Detailed Standard Parasitic Format See DSPF deviation, average 351 device model cards 27 diodes junction 160 models 160 polysilicon capacitor length 160 DSPF expansion 327 file structure 321 DTEMP parameter 352, 353 E edge condition 413 element active BJTs 162 diodes 159 JFETs 164 MESFETs 164 MOSFETs 166 C (capacitor) 123 identifiers 65 L (inductor) 130 Index F markers, mutual inductors 128 names 78 passive 113 capacitors 119 inductor 125 mutual inductor 128 R (resistor) 116 statements 72, 91 temperature 353 transmission line 140, 143 element parameters .ALTER blocks 83, 84 BJTs 162 capacitors 120 DTEMP 352 inductors 125–127 JFETs and MESFETs 164–165 linear inductors 125, 137 MOSFETs 166–168 mutual inductors, Kxxx 128 resistors 114–115 transmission lines T Element 144 W Element 140, 140–141 elements coupled inductor 134 .END statement for multiple HSPICE runs 86 in libraries 82 location 86 missing 57 with .ALTER 83, 85 .ENDL statement 81 .ENV statement 312 Envelope Analysis (ENV) 311 envelope simulation 311 .ENVFFT 314 .ENVFFT statement 314 environment variables 91 .ENVOSC 313 .ENVOSC statement 313 errors missing .END statement 57 example comment line 72 configuration file 402 Monte Carlo 365, 371 worst case 371 examples, RF tutorials 15 exp(x) function 101 exponential function 101 expressions, algebraic 99 Extended output variables 405 external data files 69 F fall time verification 413 files external data 69, 81 .hl# 305 hspice.ini 91 hspicerf 399 include files 68 .ls# 310 multiple simulation runs 86 .p2d# 310 .printhl# 305 .printls# 309 .printss# 309 .ss# 310 files, output 10 first character descriptions 63 flags 399 flush_waveform configuration option 400 format output DSPF 321 format, output NW 394 WDB 393 Foster pole-residue form E element 179 G element 179 frequency variable 104 frequency table model 153 frequency-dependent capacitor 124 inductor 130 resistor 118 functions built-in 100–104 table 100 423 Index G G GAUSS functions 366 keyword 363 parameter distribution 359 generating output 10 global parameters 105 GND node 79 ground, node name 79 ground_floating_ node configuration option 400 H Harmonic Balance (HB) 197 analysis spectrum 201 equations 199 errors 216 options 203 oscillator analysis 229 output 206 syntax 200 warnings 216 .HB for HBLIN 300 HB analysis IP3 amplifier 22 power amplifier 19 HBAC 40, 257 errors 262, 267 example 40 output 259, 315 output data files 261 syntax 258 warnings 262, 267 HBAC analysis mixer 38 .HBLIN 298, 301 limitations 300 output syntax 304 .HBLSP 305 example 308 input syntax 307 limitations 306 output data files 305, 309 output syntax 309 .HBOSC options 235 HBOSC analysis 424 Colpitts oscillator 28 VCO 31 .HBOSC statement 229 HBXF command 287 hertz variable 104 hier_delimiter configuration option 400 hierarchical designs, flattened 68 .hl# file 305 hold time verification 414 hspice.ini file 91 hspicerf command 9 hspicerf file 399 hspicerf test 400 html configuration option 400 I IBIS buffers 155 ideal transformer 137 .INCLUDE statement 68, 83, 84, 91, 93 individual element temperature 353 inductor coupled 134 frequency-dependent 130 inductors element 125 node names 125, 138 input data for data driven analysis 81 files character case 58 compression 57 netlist 57 structure 68 table of components 69 netlist 70 netlist file 70–86 input data 85 input files demonstration 55 input files, demo examples 55 int(x) function 102 integer function 102 integer_node configuration option 400 internal nodes, referencing 79 invoking HSPICE RF 9 Index J IR drop checking 415 JFETs elements 164 length 164 width 164 jitter random, with clock source 191 jitter, random, clock source 191 matrix reduction 344 resistor 116 linear elements elements, linear 139 local parameters 105 log(x) function 101 log10(x) function 101 logarithm function 101 low noise amplifier 15 .LPRINT statement 395 .ls# file 310 K M keywords DTEMP 352 MONTE 360 PAR 100 macros 85 manufacturing tolerances 367 max(x,y) function 102 max_waveform_size configuration option 400 mean, statistical 351 .measure 315 .MEASURE ENV command 315 .MEASURE statement parameters 99 MESFETs 164 min(x,y) function 102 mixer 38 model cards 27 model parameters .ALTER blocks 83, 84 capacitance distribution 369 DELVTO 355 DTEMP 353 LENGTH 368 manufacturing tolerances 367 PHOTO 368 RSH 355 sigma deviations, worst case analysis 355 skew 354 TEMP 80, 353 temperature analysis 353 TOX 355 TREF 351, 353 XPHOTO 368 .MODEL statement 353 models Monte Carlo analysis 359, 364, 371 reference temperature 353 specifying 92 J L L Element (inductor) 130 large-signal S parameter extraction 305 LENGTH model parameter 368 .LIB call statement 81 statement 68, 93 in .ALTER blocks 81, 83, 84 with .DEL LIB 85 with multiple .ALTER statements 84, 85 libraries adding with .LIB 85 ASIC cells 92 building 81 configuring 108 creating parameters 106 DDL 91 duplicated parameter names 106 .END statement 82 integrity 105 search 91 subcircuits 93 vendor 92 LIMIT keyword 363 LIN analysis 15 linear acceleration 344 capacitor 123 inductor 130 425 Index N typical set 358 Monte Carlo analysis 350, 351, 371–380 distribution options 362–363 Monte Carlo analaysis operating-point results in transient analysis 373 MONTE keyword 360 MOSFETs drain diffusion area 166 elements 166 initial conditions 167 node names 166 perimeter 167 source 167, 168 squares 167 temperature differential 167 zero-bias voltage threshold shift 168 multiple .ALTER statements 83, 84 multiply parameter 88, 115 multi-tone HB analysis mixer 38 mutual inductor 128 N natural log function 101 negative_td configuration option 401 netlist 68 file example 70 flat 68 input files 57 schematic 68 structure 70 netlist file, example 70 nodes connection requirements 79 floating supply 79 internal 79 MOSFET’s substrate 79 names 75, 80 automatic generation 80 ground node 79 period in 76 subcircuits 78, 79 numbers 75 terminators 79 noise .HBNOISE 268, 275 noise parameter extraction 426 small-signal 305 nonlinear perturbation algorithm 242 numerical integration 389, 390 NW output format 394 O operators 100 optimization 407 syntax 407 .OPTION .ALTER blocks 83, 84 MAXORD 391 PURETP 392 SIM_ACCURACY 390 SIM_DELTAI 396 SIM_DELTAV 396 SIM_DSPF 320 SIM_DSPF_ACTIVE 320, 323 SIM_DSPF_INSERROR 325 SIM_DSPF_LUMPCAPS 325 SIM_DSPF_MAX_ITER 324 SIM_DSPF_RAIL 324 SIM_DSPF_SCALEC 324 SIM_DSPF_SCALER 324 SIM_DSPF_VTOL 323 SIM_LA 320, 321, 344, 347 SIM_LA_FREQ 347 SIM_LA_MAXR 347 SIM_LA_MINC 348 SIM_LA_MINMODE 348 SIM_LA_TIME 348 SIM_LA_TOL 348 SIM_ORDER 389, 391 SIM_OSC_DETECT_TOL 392 SIM_POSTAT 404 SIM_POSTDOWN 404 SIM_POSTSCOPE 405 SIM_POSTSKIP 403, 404 SIM_POWERDC_ACCURACY 416 SIM_POWERDC_HSPICE 416 SIM_POWERPOST 418 SIM_POWERSTART 418 SIM_SPEF 320 SIM_SPEF_ACTIVE 323 SIM_SPEF_INSERROR 325 SIM_SPEF_LUMPCAPS 325 SIM_SPEF_MAX_ITER 324 Index P SIM_SPEF_PARVALUE 325 SIM_SPEF_RAIL 324 SIM_SPEF_SCALEC 324 SIM_SPEF_SCALER 324 SIM_SPEF_VTOL 323 SIM_TG_THETA 391 SIM_TRAP 391 options, configuration file 400 oscillator HB analysis 229 phase noise 238 oscillator analysis 229 oscillator example 28 output files 10 format DSPF 327 NW 394 tabulated data 393 WDB 393 generating 10 restricting 403 variables function 103 P .p2d# file 310 packed input files 57 PAR keyword 100 .PARAM statement 82, 350 in .ALTER blocks 83, 84 parameters algebraic 99, 100 analysis 99 assignment 97 cell geometry 105 constants 97 data type 97 data-driven analysis 81 defaults 108 defining 95, 106 evaluation order 97 hierarchical 88, 104 inheritance 107, 108 input netlist file 67 libraries 106–108 M 88 measurement 99 modifying 81 optimization 105 overriding 106, 108 PARHIER option 108 passing 104–111 order 97 problems 111 Release 95.1 and earlier 111 scope 104–105, 111 simple 97 subcircuit 88 user-defined 98 PARHIER option 108 passive element 113 path names 79 periodic AC algorithm 242 periodic pime-dependent noise analysis 281 phase noise 238 phase noise analysis 238 PHASENOISE 238, 240 PHASENOISE algorithms 242 PHOTO model parameter 368 PI (linear acceleration) algorithm 346 port_element_voltage_matchload configuration option 401 pow(x,y) function 101 power amplifier 19 power amplifier IP3 22 .POWER statement 417 power, function 101 .POWERDC statement 415 .PRINT ENV command 315 .printhl# file 305 .printls# file 309 .printss# file 309 .PROBE command 315 Probing Subcircuit currents 405 PTDNOISE input syntax 282 .MEASURE 286 output file format 285 output syntax 284 overview 281 syntax 282 PTDNOISE command 281 pwr(x,y) function 101 427 Index Q Q quality assurance 350 R R Element (resistor) 116 rcells, reusing 106 rcxt_divider configuration option 401 reference temperature 80, 353 reluctors 134 resistor frequency-dependent 118 length parameter 115 linear 116 model name 114 node to bulk capacitance 115 width parameter 115 restricting output 403 results 41 reusing simulation output 395, 415, 417 RF demo files 55 tutorial examples 15 rise time example 413 verify 412 RSH model parameter 355 S S parameter extraction large-signal 305 power-dependent 297 small-signal 305 saturable core elements 128 models 127, 128 scale factors 66 SCALE parameter 115 schematic netlists 68 schematic netlists 68 scope of parameters 105 SEARCH option 93 SETUP time verification 414 sgn(x) function 102 Shooting Newton driven phase frequency circuit example 43 428 overview 219 ring oscillator example 50 sign function 102 signed power function 101 silicon-on-sapphire devices 80 SIM_ACCURACY option 390 SIM_ACTIVE option 320, 323, 324, 325 SIM_DELTAI option 396 SIM_DELTAV option 396 SIM_DSPF option 320, 389, 390, 396 SIM_DSPF_ACTIVE option 320, 323 SIM_DSPF_INSERROR option 325 SIM_DSPF_LUMPCAPS option 325 SIM_DSPF_MAX_ITER option 324 SIM_DSPF_RAIL option 324 SIM_DSPF_SCALEC option 324 SIM_DSPF_SCALER option 324 SIM_DSPF_VTOL option 323 SIM_LA option 320, 321, 344, 347 SIM_LA_FREQ option 347 SIM_LA_MAXR option 347 SIM_LA_MINC option 348 SIM_LA_MINMODE option 348 SIM_LA_TIME option 348 SIM_LA_TOL option 348 SIM_ORDER option 389 SIM_POSTAT option 404 SIM_POSTDOWN option 404 SIM_POSTSCOPE option 405 SIM_POSTSKIP option 403, 404 SIM_POWERDC_ACCURACY option 416 SIM_POWERED_HSPICE option 416 SIM_POWERPOST option 418 SIM_POWERSTART option 418 SIM_SPEF option 320 SIM_SPEF_ACTIVE option 323 SIM_SPEF_INSERROR option 325 SIM_SPEF_LUMPCAPS option 325 SIM_SPEF_MAX_ITER option 324 SIM_SPEF_PARVALUE option 325 SIM_SPEF_RAIL option 324 SIM_SPEF_SCALEC option 324 SIM_SPEF_SCALER option 324 SIM_SPEF_VTOL option 323 simulation Index T multiple runs 86 title 71 simulation engine 1 sin(x) function 100 sinh(x) function 101 skew file 358 parameters 354 skip_nrd_nrs configuration option configuration options skip_nrd_nrs 401 slew rate example 412 verification 412 small-signal noise parameter extraction 305 small-signal S parameter extraction 305 SN steady-state time domain analysis 219 SNAC input syntax 263 output data files 266 SNFT 224 SNNOISE 275 input syntax 276 output data files 279 SNOSC 236 SNXF 291 source statements 72 sqrt(x) function 101 square root function 101 .ss# file 310 starting hspicerf 9 statement 313, 314 .ENV 312 .HBOSC 229 statements .AC 353 .CHECK EDGE 413 .CHECK FALL 413 .CHECK GLOBAL_LEVEL 412 .CHECK HOLD 414 .CHECK IRDROP 415 .CHECK RISE 412 .CHECK SETUP 414 .CHECK SLEW 412 .DATA 81 .DC 353 element 72 .ENDL 81 .HBXF 287 .LIB 81 .LPRINT 395 .MODEL 353 .PARAM 82 .POWER 417 .POWERDC 415 .PTDNOISE 281 source 72 .SURGE 418 .TEMP 80, 353, 354 .TRAN 353, 417 statistical analysis 354–380 statistics, calculations 351 steady state time domain analysis, Shooting Newton 219 strobejitter 286 subcircuit probing currents 405 subcircuits calling tree 79 changing in .ALTER blocks 82, 84 creating reusable circuits 87 hierarchical parameters 88 library structure 93 multiplying 89 node names 78 path names 79 .PRINT and .PLOT statements 90 .SURGE statement 418 T tabulated data output 393 Taguchi analysis 350 tan(x) function 100 tanh(x) function 101 TEMP model parameter 80, 353 .TEMP statement 353, 354 temper variable 104 temperature circuit 351, 353 coefficients 115 derating 80, 353 element 353 reference 80, 353 429 Index U variable 104 Temperature Variation Analysis 350 time domain steady state analysis 219 time variable 104 title for simulation 71 .TITLE statement 71 TNOM option 80, 353 TOX model parameter 355 .TRAN statement 353, 417 transfer sign function 102 transformer, ideal 137 Trapezoidal (TRAP) integration algorithm 389, 390 TREF model parameter 353 tutorial 15 overview 1 simulation engine 1 two-tone HB 39 U UNIF keyword 363 uniform parameter distribution 359 unit_atto configuration option 401 V v_supply configuration option 401 variables changing in .ALTER blocks 82, 84 HSPICE-specific 104 variance, statistical 351 VCD format 393 VCO 31 vector-modualted RF 180 vector-modulated RF E element 186 F element 186 430 G element 186 H element 186 I element 182 implementation 180 V element 182 vendor libraries 92 VMRF, See vector-modulated RF 180 Vnn node name in CSOS 80 W warnings floating power supply nodes 79 waveform display 12 WDB format 393 W-elements 140 wildcard uses 76, 402 wildcard_left_range configuration option 401 wildcard_match_all configuration option 402 wildcard_match_one configuration option 402 wildcard_right_range configuration option 402 worst case analysis 354, 371, 380 Worst Case Corners Analysis 350 X X() variable 405 XL model parameter 355 XPHOTO model parameter 368 XW model parameter 355 Y yield analysis 350

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

Download PDF

advertisement