Synopsys HSPICE USER MANUAL

HSPICE® Signal Integrity User Guide

Version X-2005.09, September 2005

Copyright  2005 Syno psys, Inc. All rights reserved. This softw are and documentation con tain confidential and prop rietary information that is the property of Synopsys, Inc. The softwar e and documentation are furnished under a license ag reement 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 em ployees. This is copy number __________.”

Destination Control Statement

All technical data contained in this publication is subject to the export control laws of the United States of America. Disclosure to nationals of other countries contrary to United States law is prohibited. It is the reader’s responsibility to determine the applicable regulations and to comply with them.

Disclaimer

SYNOPSYS, INC., AND ITS LICENSORS MAKE NO WARRANTY OF ANY KIND, EXPRESS OR IMPLIED, WITH REGARD TO THIS MATERIAL, INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE.

Registered Trademarks (®)

Synopsys, AMPS, Arcadia, C Level Design, C2HDL, C2V, C2VHDL, Cadabra, Calaveras Algorithm, CATS, CRITIC, CSim, Design Compiler, DesignP ow er , DesignW are, EPIC , F ormality, HSIM, HSPICE, Hypermodel, iN-Phase, in-Sync, Leda, MAST , Meta, Meta-Software, ModelT ools, NanoSim, OpenVera, P athMill, Photolynx, Physical Compiler, Po werMill, PrimeTime, RailMill, RapidScript, Saber, SiVL, SNUG, SolvNet, Superlog, System Compiler, T estify , TetraMAX, TimeMill, TMA, VCS, Vera, and Virtual Stepper are registered trademarks of Synopsys, Inc.

Trademarks (™)

Active Parasitics, AFGen, Apollo, Apollo II, Apollo-DPII, Apollo-GA, ApolloGAII, Astro, Astro-Rail, Astro-Xtalk, Aurora, AvanTestchip, AvanWaves, BCView, Behavioral Compiler, BOA, BRT, Cedar, ChipPlanner, Circuit Analysis, Columbia, Columbia-CE, Comet 3D, Cosmos, CosmosEnterprise, CosmosLE, CosmosScope, CosmosSE, Cyclelink, Davinci, DC Expert, DC Expert Plus, DC Professional, DC Ultra, DC Ultra Plus, Design Advisor, Design Analyzer, Design Vision, DesignerHDL, DesignTime, DFM-Workbench, Direct RTL, Direct Silicon Access, Discovery, DW8051, DWPCI, Dynamic-Macromodeling, Dynamic Model Switcher, ECL Compiler, ECO Compiler , EDAna vigator , Encore, Encore PQ, Evaccess, ExpressModel, Floorplan Manager, Formal Model Checker , FoundryModel, FPGA Compiler II, FPGA Express, Frame Compiler, Galaxy, Gatran, HANEX, HDL Advisor, HDL Compiler, Hercules, Hercules-Explorer, Hercules-II,

Hierarchical Optimization Technology, High Performance Option, HotPlace, HSIM Integrator, Interactive Waveform Viewer, i-Virtual Stepper, Jupiter, Jupiter-DP, JupiterXT, JupiterXT-ASIC, JVXtreme, Liberty, Libra-Passport, Library Compiler, Libra-Visa, Magellan, Mars, Mars-Rail, Mars-Xtalk, Medici, Metacapture, Metacircuit, Metamanager, Metamixsim, Milkywa y, ModelSource, Module Compiler, MS-3200, MS-3400, Nova Product Family, Nova-ExploreRTL, Nova-Trans, Nova-VeriLint, Nova-VHDLlint, Optimum Silicon, Orion_ec, Parasitic View, Passport, Planet, Planet-PL, Planet-RTL, Polaris, Polaris-CBS, Polaris-MT, Power Compiler, PowerCODE, PowerGate, ProFPGA, ProGen, Prospector, Protocol Compiler, PSMGen, Raphael, Raphael-NES, RoadRunner, RTL Analyzer, Saturn, ScanBand, Schematic Compiler, Scirocco, Scirocco-i, Shadow Debugger , Silicon Blueprint, Silicon Early Access, SinglePass-SoC, Smart Extraction, SmartLicense, SmartModel Library , Softwire, Source-Level Design, Star, Star-DC, Star-MS, Star-MTB, Star-Power, Star-Rail, Star-RC, Star-RCXT, Star-Sim, Star-SimXT, Star-Time, Star-XP, SWIFT, Taurus, TimeSlice, TimeTracker, Timing Annotator, TopoPlace, TopoRoute, Trace-On-Demand, True-Hspice, TSUPREM-4, TymeWare, VCS Express, VCSi, Venus, Verification Portal, VFormal, VHDL Compiler, VHDL System Simulator, VirSim, and VMC are trademarks of Synopsys, Inc.

Service Marks (SM)

MAP-in, SVP Café, and TAP-in are ser vice marks of Synopsys, Inc.

plus

, HSPICE-Link, iN-Tandem,

SystemC is a trademark of the Open SystemC Initiative and is used under license. ARM and AMBA are registered trademarks of ARM Limited. All other product or company names may be trademarks of their respective owners.

Printed in the U.S.A. HSPICE

Signal Integrity User Guide, X-2005.09

ii HSPICE® Signal Integrity User Guide

X-2005.09

Inside This Manual. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xi

The HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xii

Searching Across the HSPICE Documentation Set. . . . . . . . . . . . . . . . . . . . . xiii

Other Related Publications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xiv

Conventions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xiv

Customer Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . xv

1. Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1

Preparing for Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1

Signal Integrity Problems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

Analog Side of Digital Logic . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

Optimizing TDR Packaging . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

Using TDR in Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

TDR Optimization Procedure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10

Simulating Circuits with Signetics Drivers . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

Simulating Circuits with Xilinx FPGAs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

Syntax for IOB (xil_iob) and IOB4 (xil_iob4) . . . . . . . . . . . . . . . . . . . . . . 17

Ground-Bounce Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18

Coupled Line Noise . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20

2. S Parameter Modeling Using the S Element . . . . . . . . . . . . . . . . . . . . . . . . 25

S Parameter Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25

Using the Scattering Parameter Element. . . . . . . . . . . . . . . . . . . . . . . . . 26

S Element Syntax. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27

S Model Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32

S Element Data File Model Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . 35

S Element Noise Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38

HSPICE® Signal Integrity User Guide iii X-2005.09

Contents

Two-Port Noise Parameter Support in Touchstone Files . . . . . . . . . 38

Input Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39

Output Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40

Notifications and Limitations. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41

Multiport Noise Model for Passive Systems. . . . . . . . . . . . . . . . . . . . . . . 41

Input Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41

Output Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43

Notifications and Limitations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43

Mixed-Mode S Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44

Relating Voltage and Current Waves to Nodal Waves. . . . . . . . . . . . . . . 44

Characterizing Differential Data Transfer Systems. . . . . . . . . . . . . . . . . . 46

Deriving a Simpler Set of Voltage and Current Pairs. . . . . . . . . . . . . . . . 46

Using the Mixed-Mode S Parameters (S Element) . . . . . . . . . . . . . . . . . 48

Mixed-Mode S Parameter Netlist Examples. . . . . . . . . . . . . . . . . . . 50

Small-Signal Parameter Data-Table Model . . . . . . . . . . . . . . . . . . . . . . . . . . . 50

SP Model Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50

3. Modeling Coupled Transmission Lines

Using the W Element. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .61

Equations and Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 62

Frequency-Dependent Matrices. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63

Determining Matrix Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64

Wave Propagation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65

Propagating a Voltage Step . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 67

Handling Line-to-Line Junctions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69

Using the W Element. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70

Control Frequency Range of Interest for Greater Accuracy. . . . . . . . . . . 71

.OPTION RISETIME Setting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 72

Use DELAYOPT Keyword for Higher Frequency Ranges. . . . . . . . . 72

Use DCACC Keyword for Lower Frequency Ranges . . . . . . . . . . . . 73

W Element Time-Step Control in Time Domain. . . . . . . . . . . . . . . . . . . . 73

Using Static Time-Step Control . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73

Using Dynamic Time-Step Control. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73

Input Syntax for the W Element . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75

Input Model 1: W Element, RLGC Model. . . . . . . . . . . . . . . . . . . . . . . . . 78

Specifying the RLGC Model in an External File. . . . . . . . . . . . . . . . 82

Input Model 2: U Element, RLGC Model . . . . . . . . . . . . . . . . . . . . . . . . . 84

Using RLGC Matrices. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 85

Input Model 3: Built-in Field-Solver Model . . . . . . . . . . . . . . . . . . . . . . . . 88

iv HSPICE® Signal Integrity User Guide

X-2005.09

Contents

Input Model 4: Frequency-Dependent Tabular Model . . . . . . . . . . . . . . . 88

Notation Used. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89

Table Model Card Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 89

SP.MODEL Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90

Input Model 5: S Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92

S Model Conventions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93

S Model Example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 94

Extracting Transmission Line Parameters (Field Solver) . . . . . . . . . . . . . . . . . 94

Filament Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95

Modeling Geometries. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96

Solver Limitation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96

Field-Solver Statement Syntax. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96

Defining Material Properties. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97

Creating Layer Stacks . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97

Defining Shapes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97

Field-Solver Options. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97

Using the Field Solver Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97

Field Solver Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99

Example 1: Cylindrical Conductor Above a Ground Plane. . . . . . . . 99

Example 2: Stratified Dielectric Media . . . . . . . . . . . . . . . . . . . . . . . 102

Example 3: Two Traces Between Two Ground Planes . . . . . . . . . . . 104

Example 4: Using Field Solver with Monte Carlo Analysis. . . . . . . . 106

W Element Passive Noise Model. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109

Input Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109

Output Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 112

List of Transmission Line Models. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113

4. Modeling Input/Output Buffers Using IBIS . . . . . . . . . . . . . . . . . . . . . . . . . 117

Verifying IBIS Files with the Golden Parser . . . . . . . . . . . . . . . . . . . . . . . . . . . 118

Using Buffers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 118

IBIS Conventions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119

Terminology . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 120

Buffers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121

Input Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121

Output Buffer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123

Tristate Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126

Input/Output Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 129

Open Drain, Open Sink, Open Source Buffers . . . . . . . . . . . . . . . . . . . . 132

I/O Open Drain, I/O Open Sink, I/O Open Source Buffers. . . . . . . . . . . . 132

HSPICE® Signal Integrity User Guide v X-2005.09

Contents

Input ECL Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 133

Output ECL Buffer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134

Tristate ECL Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135

Input-Output ECL Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 137

Terminator Buffer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 138

Series Buffer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141

Series Switch Buffer. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141

Multilingual Model Support. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 143

Specifying Common Keywords . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 144

Optional Keywords. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 144

file. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145

model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145

buffer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145

typ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 147

hsp_ver . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 148

power . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149

interpol . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149

xv_pu | xv_pd. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150

ramp_fwf | ramp_rwf . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151

fwf_tune | rwf_tune. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151

rwf_pd_dly | fwf_pu_dly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153

ss_state . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154

nowarn . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154

Differential Pins . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156

Buffers in Subcircuits. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157

Netlist Example with Output Buff er, Transmission Line, and Input Buffer . . . . 159

Using the IBIS Buffer Component . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160

Required Keywords . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160

file=’file_name’ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160

component=’component_name’. . . . . . . . . . . . . . . . . . . . . . . . . . . . 161

Optional Keywords. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 161

package . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 161

pkgfile=’pkg_file_name’ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162

Other Optional Keywords . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162

Component Calls for SPICE-Formatted Pins . . . . . . . . . . . . . . . . . . . . . . 163

How.IBIS Creates Buffers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163

Using the Buffer Component . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164

Buffer Power ON. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164

vi HSPICE® Signal Integrity User Guide

X-2005.09

Contents

Buffer Power OFF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168

.IBIS Command . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 172

Using IBIS Board-Level Components . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 173

.EDB and .IBIS Command Syntax . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 175

Circuit Topology Created by the .EBD and .IBIS Commands. . . . . . . . . . 177

B Element Naming Rules. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 178

IBIS Board-Level Component Examples . . . . . . . . . . . . . . . . . . . . . . . . . 181

Nodes Used with B Elements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 182

Additional Notes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 183

Keywords . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 183

Voltage Thresholds . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 183

.OPTION D_IBIS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 184

Subcircuit Model. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 184

Driver Schedule . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 184

5. Modeling Ideal and Lumped Transmission Lines . . . . . . . . . . . . . . . . . . . . 185

Selecting Wire Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186

Source Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187

Interconnect Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187

Using Ground and Reference Planes . . . . . . . . . . . . . . . . . . . . . . . . . . . 189

Selecting Ideal or Lossy T ransmission Line Element. . . . . . . . . . . . . . . . 189

Selecting U Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 191

Transmission Lines: Example. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 192

Interconnect Simulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 193

Ideal Transmission Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 193

Lossy U Element Statement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 194

Lossy U Model Statement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 195

Planar Geometric Models Lossy U Model Parameters . . . . . . . . . . . . . . 197

Common Planar Model Parameters. . . . . . . . . . . . . . . . . . . . . . . . . 197

Physical Parameters. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199

Loss Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 199

Geometric Parameter Recommended Ranges . . . . . . . . . . . . . . . . 200

Reference Planes and HSPICE Ground . . . . . . . . . . . . . . . . . . . . . 201

Estimating the Skin Effect Frequency. . . . . . . . . . . . . . . . . . . . . . . . 202

Number of Lumped-Parameter Sections . . . . . . . . . . . . . . . . . . . . . 203

Ringing. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 203

Geometric Parameters (ELEV=1). . . . . . . . . . . . . . . . . . . . . . . . . . . 204

Lossy U Model Par ameters for Geometric Coax (PLEV=2, ELEV=1) . . . 208

HSPICE® Signal Integrity User Guide vii X-2005.09

Contents

Lossy U Model Parameters Geometric Twinlead (PLEV=3, ELEV=1) . . . 210

Precomputed Model Parameters (ELEV=2). . . . . . . . . . . . . . . . . . . 212

Conductor Width Relative to Reference Plane Width. . . . . . . . . . . . 215

Alternative Multi-conductor Capacitance/Conductance Definitions . 215

Measured Parameters (ELEV=3) . . . . . . . . . . . . . . . . . . . . . . . . . . . 218

U Element Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 220

Three Coupled Lines, Stripline Configuration. . . . . . . . . . . . . . . . . . 220

Three Coupled Lines, Sea of Dielectric Configuration . . . . . . . . . . . 225

Simulation Output. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 229

IcWire Output Section . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 230

Capacitance and Inductance Matrices. . . . . . . . . . . . . . . . . . . . . . . 232

Five Coupled Lines, Stripline Configuration . . . . . . . . . . . . . . . . . . . 234

U Model Applications . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 235

Data Entry Examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 235

Printed Circuit Board Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 236

Coax Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 237

Twinlead Models. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 238

Two Coupled Microstrips . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 238

Solving Ringing Problems with U Elements. . . . . . . . . . . . . . . . . . . . . . . 240

Oscillations Due to Simulation Errors. . . . . . . . . . . . . . . . . . . . . . . . 240

Timestep Control Error. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 240

Incorrect Number of Element Lumps . . . . . . . . . . . . . . . . . . . . . . . . 240

Default Computation. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 241

Using a Multi-stage RC Filter to Prevent Ringing. . . . . . . . . . . . . . . 242

Signal Reflections Due to Impedance Mismatch . . . . . . . . . . . . . . . 244

Transmission Line Theory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 246

Lossless Transmission Line Model. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 247

Lossy Transmission Line Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 247

Impedance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 248

Impedance of Simple Lumped Elements . . . . . . . . . . . . . . . . . . . . . 249

Characteristic Impedance. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 250

Inductance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 251

Mutual Inductance and Self Inductance. . . . . . . . . . . . . . . . . . . . . . 251

Operational Definition of Inductance . . . . . . . . . . . . . . . . . . . . . . . . 251

Mutual Inductance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 252

Self Inductance. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253

Reference Plane Return Paths. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253

Crosstalk in Transmission Lines. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 254

Risetime, Bandwidth, and Clock Frequency. . . . . . . . . . . . . . . . . . . . . . . 255

Definitions of Transmission Line Terms . . . . . . . . . . . . . . . . . . . . . . . . . . 256

Relationships and Rules of Thumb . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 258

Time and Frequency Relationships . . . . . . . . . . . . . . . . . . . . . . . . . 258

Transmission Line Effects. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 259

viii HSPICE® Signal Integrity User Guide

X-2005.09

Contents

Intrinsic Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 259

Reflections . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 260

Loss and Attenuation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 261

Physical Design Quantities. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 262

Attenuation in Transmission Lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 263

Physical Basis of Loss . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 264

Skin Depth . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 265

Dielectric Loss . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 266

Lossy Transmission Line Model . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 267

Attenuation Due to Conductor Resistance. . . . . . . . . . . . . . . . . . . . 268

Attenuation Due to the Dielectric . . . . . . . . . . . . . . . . . . . . . . . . . . . 269

Integrating Attenuation Effects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 269

References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 270

Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271

HSPICE® Signal Integrity User Guide ix X-2005.09

Contents

xHSPICE

Signal Integrity User Guide

X-2005.09

This manual describes how to use HSPICE to maintain signal integrity in your chip design.

Inside This Manual

This manual contains the chapters described below. For descriptions of the other manuals in the HSPICE documentation set, see the next section, “The

HSPICE Documentation Set.”

Chapter Description

Chapter 1, Introduction Describes some of the factors that can affect

About This Manual

signal integrity in your design.

Chapter 2, S Parameter Modeling Using the S Element

Chapter 3, Modeling Coupled Transmission Lines Using the W Element

HSPICE® Signal Integrity User Guide xi X-2005.09

Describes S parameter and SP modeling as well as other topics related to the S element

Describes how to use basic transmission line simulation equations and an optional method for computing the parameters of transmission line equations.

About This Manual

The HSPICE Documentation Set

Chapter Description

Chapter 4, Modeling Input/ Output Buffers Using IBIS

Chapter 5, Modeling Ideal and Lumped Transmission Lines

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 model input and output buffe rs using IBIS. Includes information on IBIS conventions , buf fers , and the IBIS golden parser .

Describes how to model ideal and lumped transmission lines.

Describes how to use HSPICE to simulate and analyze your circuit designs. This is the main HSPICE user guide.

HSPICE Signal Integrity Guide

HSPICE Applications Manual

HSPICE Command Reference

HPSPICE Elements and Device Models Manual

Describes how to use HSPICE to maintain signal integrity in your chip design.

Provides application examples and additional HSPICE user information.

Provides reference information for HSPICE commands.

Describes standard models you can use when simulating your circuit designs in HSPICE, including passive devices, diodes, JFET and MESFET devices, and BJT devices.

HPSPICE MOSFET Models Manual

Describes standard MOSFET models you can use when simulating your circuit designs in HSPICE.

xii HSPICE® Signal Integrity User Guide

X-2005.09

About This Manual

Searching Across the HSPICE Documentation Set

Manual Description

HSPICE RF Manual Describes a special set of analysis and design

capabilities added to HSPICE to support RF and high-speed circuit design.

AvanWaves User Guide Describes the AvanWaves tool, which you can

use to display waveforms generated during HSPICE circuit design simulation.

HSPICE Quick Reference Guide

HSPICE Device Models Quick Reference Guide

Provides key reference information for using HSPICE, including syntax and descriptions for commands, options, paramete rs, elements, and more.

Provides key reference information for using HSPICE device models, including passive devices, diodes, JFET and MESFET devices, and BJT devices.

Searching Across the HSPICE Documentation Set

Synopsys includes an index with your HSPICE documentation that lets you search the entire HSPICE documentation set for a particular topic or keyword. In a single operation, you can instantly generate a list of hits that are hyperlinked to the occurrences of your search term. For information on how to perform searches across multiple PDF documents, see the HSPICE release notes (available on SolvNet at http://solvnet.synopsys.com) or the Adobe Reader online help.

Note: To use this feature, the HSPICE documentation files, the Inde x 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.

HSPICE® Signal Integrity User Guide xiii X-2005.09

About This Manual

Other Related Publications

For additional information about HSPICE, see:

■

The HSPICE release notes, available on SolvNet (see Accessing SolvNet

on page xv)

■

Documentation on the Web, which provides PDF documents and is available through SolvNet at http://solvnet.synopsys.com

■

The Synopsys MediaDocs Shop, from which you can order printed copies of Synopsys documents, at http://mediadocs.synopsys.com

You might also want to refer to the documentation for the following related Synopsys products:

■

CosmosScope

■

Aurora

■

Raphael

■

VCS

Conventions

The following conventions are used in Synopsys documentation.

Convention Description

Courier Indicates command syntax.

Italic

Bold Indicates user input—text y ou type verbatim—in syntax and

[ ] Denotes optional parameters, such as

...

Indicates a user-defined value, such as object_name.

examples.

write_file [-f filename]

Indicates that a parameter can be repeated as many times as necessary:

pin1 [pin2 ... pinN]

xiv HSPICE® Signal Integrity User Guide

X-2005.09

Convention Description

| Indicates a choice among alternatives, such as

\ Indicates a continuation of a command line. / Indicates levels of directory structure. Edit > Copy Indicates a path to a menu command, such as opening the

Control-c Indicates a keyboard combination, such as holding down

Customer Support

About This Manual

Customer Support

low | medium | high

Edit menu and choosing Copy.

the Control key and pressing c.

Customer support is available through SolvNet online customer support and through contacting the Synopsys Technical Support Center.

Accessing SolvNet

SolvNet includes an electronic knowledge base of technical articles and answers to frequently asked questions about Synopsys tools. SolvNet also gives you access to a wide range of Synopsys online services, which include downloading software, viewing Documentation on the Web, and entering a call to the Support Center.

To access SolvNet,

1. Go to the SolvNet Web page at http://solvnet.synopsys.com.

2. If prompted, enter your user name and password. (If you do not have a Synopsys user name and password, follow the instructions to register with SolvNet.)

If you need help using SolvNet, click SolvNet Help in the Support Resources section.

HSPICE® Signal Integrity User Guide xv X-2005.09

About This Manual

Customer Support

Contacting the Synopsys Technical Support Center

If you hav e prob lems, questions , or suggestions, y ou can contact the Synopsys Technical Support Center in the following ways:

■

Open a call to your local support center from the Web by going to

http://solvnet.synopsys.com (Synopsys user name and passw ord required),

then clicking “Enter a Call to the Support Center.”

■

Send an e-mail message to your local support center.

• E-mail support_center@synopsys.com from within North America.

• Find other local support center e-mail addresses at

■

Telephone your local support center.

• Call (800) 245-8005 from within the continental United States.

• Call (650) 584-4200 from Canada.

http://www.synopsys.com/support/support_ctr.

• Find other local support center telephone numbers at

http://www.synopsys.com/support/support_ctr.

xvi HSPICE® Signal Integrity User Guide

X-2005.09

Describes some of the factors that can affect signal integrity in your design.

The performance of an IC design is no longer limited to how many million transistors a vendor fits on a single chip. With tighter packaging space and increasing clock frequencies, packaging issues and system-level performance issues (such as crosstalk and transmission lines) are becoming increasingly significant. At the same time, the popularity of multi-chip packages and increased I/O counts is forcing package design to become more like chip design.

Preparing for Simulation

1Introduction

To simulate a PC board or backplane, you must model the following components:

■

Driver cell, including parasitic pin capacitances and package lead inductances.

■

Transmission lines.

HSPICE® Signal Integrity User Guide 1 X-2005.09

1: Introduction

Preparing for Simulation

■

A receiver cell with parasitic pin capacitances and package lead inductances.

■

Terminations or other electrical elements on the line.

Model the transmission line as closely as possible— that is, to maintain the integrity of the simulation, include all electrical elements exactly as they are laid out on the backplane or printed circuit board.

You can use readily-available I/O drivers from ASIC vendors, and the HSPICE device models adv anced lossy transmission lines to simulate the electrical behavior of the board interconnect, bus, or bac kplane. You can also analyz e the transmission line behavior under various conditions.

You can simulate because the critical models and simulation technology exist.

■

Many manufa cturers of high-speed components already use Synopsys HSPICE.

■

You can hide the complexity from the system level.

■

HSPICE or HSPICE RF preserves the necessary electrical characteristics with full transistor-level library circuits.

HSPICE or HSPICE RF can simulate systems by using:

■

System-lev el behavior, such as local component temperature and independent models to accurately predict electrical behavior.

■

Automatic inclusion of library components by using the SEARCH option.

■

Lossy transmission line models that:

• Support common-mode simulation.

• Include ground-plane reactance.

• Include resistive loss of conductor and ground plane.

• Allow multiple signal conductors.

• Require minimum CPU computation time.

2HSPICE

Signal Integrity User Guide

X-2005.09

1: Introduction

Preparing for Simulation

Signal Integrity Problems

Table 1 lists some of the signal integrity problems that can cause failures in high-speed designs.

Table 1 High-Speed Design Problems and Solutions

Signal Integrity Problem

Noise: delta I (current)

Noise: coupled (crosstalk)

Noise: reflective Impedance mismatch. Reduce the number of

Delay: path length

Propagation speed

Causes Solution

Multiple simultaneouslyswitching drivers; highspeed devices create larger delta I.

Closely-spaced parallel traces.

Poor placement and routing; too many or too few layers; chip pitch.

Dielectric medium. Choose the dielectric with the

Adjust or evaluate location, size, and v alue of decoupling capacitors.

Establish design rules for lengths of parallel lines.

connectors, and select proper impedance connectors.

Choose MCM or other highdensity packaging technology.

lowest dielectric constant.

Delay: rise time degradation

Resistive loss and impedance mismatch.

Adjust width, thickness, and length of line.

Analog Side of Digital Logic

Circuit simulation of a digital system becomes necessary only when the analog characteristics of the digital signals become electrically important. Is the digital circuit a new design or simply a fast v ersion of the old design? Many ne w digital products are actually faster versions of existing designs. For example, the transition from a 100 MHz to a 150 MHz Pentium PC might not require extensive logic simulations. However, the integrity of the digital quality of the signals might require careful circuit analysis.

HSPICE® Signal Integrity User Guide 3 X-2005.09

1: Introduction

Preparing for Simulation

The source of a signal integrity problem is the digital output driver. A highspeed digital output driver can drive only a few inches before the noise and delay (because of the wiring) become a problem. To speed-up circuit simulation and modeling, you can create analog behavioral models, which mimic the full analog characteristics at a fraction of the traditional evaluation time.

The roadblocks to successful high-speed digital designs are noise and signal delays. Digital noise can originate from several sources. The fundamental digital noise sources are:

■

Line termination noise—additional voltage reflected from the load back to the driver, which is caused by an impedance mismatch. Digital output buffers are not designed to accurately control the output impedance. Most buff ers have different rising and falling edge impedances.

■

Ground bounce noise—noise generated where leadframes or other circuit wires cannot form into transmission lines. The resulting inductance creates an induced voltage in the ground circuit, supply circuit, and output driver circuit. Ground bounce noise lowers the noise margins for the rest of the system.

■

Coupled line noise—noise induced from lines that are physically adjacent. This noise is generally more sev ere for data lines that are ne xt to clock lines .

Simulating the output buffer in Figure 1 demonstrates the analog behavior of a digital gate circuit or HSPICE RF.

4HSPICE

Signal Integrity User Guide

X-2005.09

1: Introduction

Preparing for Simulation

Figure 1 Simulating Output Buffer with 2 ns Delay and 1.8 ns Rise/F all Times

vdd

100.0M

-100.0M

Volt [Amp]

4.0

2.0

4.0

2.0 0

Out

Ground noise

5.0N

Ground Current

VDD Current

10.0N 15.0N 20.0N0

Time [Lin]

ACL.TRO OUT

ACL.TRO I-

I-

ACL.TRO XIN.V.LOCAL

XIN.V.LOCAL

Circuit delays become critical as timing requirements become tighter. The key circuit delays are:

■

Gate delays.

■

Line turnaround delays for tristate buffers.

■

Line length delays (clock skew).

Logic analysis addresses only gate delays. You can compute the variation in the gate delay from a circuit simulation only if you understand the best case and worst case manufacturing conditions.

The line turnaround delays add to the gate delays so you must add an extra margin that multiple tristate buffer drivers do not

simultaneously turn on. In most systems, the line-length delay most directly affects the clock skew.

As system cycle times approach the speed of electromagnetic signal propagation for the printed circuit board, consideration of the line length

HSPICE® Signal Integrity User Guide 5 X-2005.09

1: Introduction

Preparing for Simulation

becomes critical. The system noises and line delays interact with the electrical characteristics of the gates, and might require circuit level simulation.

Analog details find digital systems problems. Exceeding the noise quota might not cause a system to fail. Maximum noise becomes a problem only when HSPICE accepts a digital input. If a digital systems engineer can decouple the system, HSPICE or HSPICE RF can accept a much higher level of noise.

Common decoupling methods are:

■

Multiple ground and power planes on the PCB, MCM, and PGA.

■

Separating signal traces with ground traces.

■

Decoupling capacitors.

■

Series resistors on output buffer drivers.

■

Twisted-pair line driving.

In present systems designs, you must select the best packaging methods at three levels:

■

printed circuit board

■

multi-chip module

■

pin grid array

Extra ground and power planes are often necessary to lower the supply inductance and to provide decoupling.

■

Decoupling capacitors must have very low internal inductance to be effective for high-speed designs.

■

Newer designs frequently use series resistance in the output drivers to lower circuit ringing.

■

Critical high-speed driver applications use twisted differential-pair transmission lines.

A systems engineer must determine how to partition the logic. The propagation speed of signals on a printed circuit board is about 6 in/ns. As digital designs become faster, wiring interconnects become a factor in how you partition logic.

Note: HSPICE RF partitioning is for Operating Point (OP) only.

6HSPICE

Signal Integrity User Guide

X-2005.09

1: Introduction

Preparing for Simulation

The critical wiring systems are:

■

IC-level wiring.

■

Package wiring for SIPs, DIPs, PGAs, and MCMs.

■

Printed circuit-board wiring.

■

Backplane and connector wiring.

■

Long lines – power, coax, or twisted pair.

If you use ASIC or custom integrated circuits as part of your system logic partitioning strategy, you must make decisions about integrated circuit level wiring. The more-familiar decisions involve selecting packages and arranging packages on a printed circuit board. Large systems generally have a central backplane, which becomes the primary challenge at the system partition level.

Use the following equation to estimate wire length when transmission line effects become noticeable:

critical length=(rise time)*velocity/8

For example, if rise time is 1 ns and board velocity is 6 in/ns, then distortion becomes noticeable when wire length is 3/4 in. The HSPICE or HSPICE RF circuit simulator automatically generates models f or each type of wire to define effects of full loss transmission lines.

To partition a system, ECL logic design engineers typically used to calculate the noise quota for each line. Now, you must design most high-speed digital logic with respect to the noise quota so that the engineer knows how much noise and delay are acceptable before timing and logic levels fail.

To solve the noise quota problem, you must calculate the noise associated with the wiring. You can separate large integrated circuits into two parts:

■

Internal logic.

■

External input and output amplifiers.

When you use mixed digital and analog tools, you can merge a complete system together with full analog-quality timing constraints and full digital representation. You can simultaneously evaluate noise-quota calculations, subject to system timing.

HSPICE® Signal Integrity User Guide 7 X-2005.09

1: Introduction

Optimizing TDR Packaging

Figure 2 Analog Drivers and Wires

Optimizing TDR Packaging

Packaging plays an important role in determining the overall speed, cost, and reliability of a system. With today’s small feature sizes, and high levels of integration, a significant portion of the total delay is the time required for a signal to travel between chips.

Logic

Multi-layer ceramic technology has proven to be well suited for high-speed GaAs IC packages.

A multi-chip module (MCM) minimizes the chip-to-chip spacing. It also reduces the inductive and capacitive discontinuity between the chips mounted on the substrate. An MCM uses a more direct path (die-bump-interconnect-b ump-die), which eliminates wire bonding. In addition, narrower and shorter wires on the ceramic substrate hav e m uch less capacitance and inductance , than PC board interconnections have.

Time domain reflectometry (TDR) is the closest measurement to actual digital component functions. It provides a transient display of the impedance versus time for pulse behavior.

Using TDR in Simulation

When you use a digitized TDR file, you can use the HSPICE or HSPICE RF optimizer to automatically select design components. To extract critical points from digitized TDR files, use the .MEASURE statement, and use the results as electrical specifications for optimization. This process eliminates recurring design cycles to find component values that curve-fit the TDR files.

8HSPICE

Signal Integrity User Guide

X-2005.09

Figure 3 Optimization Process

1: Introduction

Optimizing TDR Packaging

Measure

TDR Files

Measure

Results

HSPICE

Optimization

Input File

Compare with

Actual TDR

Files

Figure 4 General Method for TDR Optimization

Pulse Generation

Oscilloscope

Test Circuit

Use the following method for realistic high-speed testing of packaging:

■

Test fixtures closely emulate a high-speed system environment.

■

A HSPICE device model uses ideal transmission lines and discrete components for measurements.

The tested circuit contains the following components:

■

Signal generator.

■

Coax connecting the signal generator to ETF (engineering test fixture) board.

■

ETF board.

■

Package pins.

■

Package body.

HSPICE® Signal Integrity User Guide 9 X-2005.09

1: Introduction

Optimizing TDR Packaging

Figure 5 SPICE Model for Package-Plus-Test Fixture

The package tests use a digital sampling oscilloscope to perform traditional time-domain measurements. Use these tests to observe the reflected and transmitted signals. These signals are derived from the built-in high-speed pulse generator and translated output signals into digitized time-domain reflectometer files (voltage versus time).

Optimized Pa rameters: XTD, CSMA, LPIN, and LPK

Use a fully-developed SPICE model to simulate the package-plus-test fixture, then compare the simulated and measured reflected/transmitted signals.

The next section shows the input netlist file for this experiment. Figure 6 through Figure 9 show the output plots.

TDR Optimization Procedure

The sample netlist for this experiment is located in the following directory:

$installdir/demo/hspice/si/ipopt.sp

10 HSPICE® Signal Integrity User Guide

X-2005.09

Figure 6 Reflected Signals Before Optimization

1: Introduction

Optimizing TDR Packaging

Simulated

Measured

Figure 7 Reflected Signals After Optimization

Simulated

Measured

HSPICE® Signal Integrity User Guide 11 X-2005.09

1: Introduction

Optimizing TDR Packaging

Figure 8 Transmitted Signals Before Optimization

Simulated

Measured

Figure 9 Transmitted Signals after Optimization

Simulated

Measured

12 HSPICE® Signal Integrity User Guide

X-2005.09

Simulating Circuits with Signetics Drivers

HSPICE or HSPICE RF includes a Signetics I/O buffer library in the $installdir/parts/signet directory. You can use these highperformance parts in backplane design. Transmission line models describe two conductors.

Figure 10 Planar Transmission Line DLEV=2: Microstrip Sea of Dielectric

Upper Ground Plane

Insulator

SP12

(5 mil)

WD1=8 mil

line 1

TH1=1.3 mil

WD1=8 mil

line 1

1: Introduction

Simulating Circuits with Signetics Drivers

TS=32 mil

TH1=1.3 mil

W1eff (6 mil)

Lower Ground Plane

HT1=10 mil

In the following application, a pair of drivers are driving about 2.5 inches of adjacent lines to a pair of receivers that drive about 4 inches of line.

HSPICE® Signal Integrity User Guide 13 X-2005.09

1: Introduction

Simulating Circuits with Signetics Drivers

Figure 11 I/O Drivers/Receivers with Package Lead Inductance, Parallel 4"

Lossy Microstrip Connectors

driver receiver

vin

An example package inductance:

LIN_PIN IN IN1 PIN_IN LOUT_PIN OUT1 OUT PIN_OUT LVCC VCC VCC1 PIN_VCC LGND XGND1 XGND PIN_GND .ENDS $ TLINE MODEL - 2 SIGNAL CONDUCTORS WITH GND $ PLANE

.MODEL USTRIP U LEVEL=3 ELEV=1 PLEV=1 + TH1=1.3mil HT1=10mil TS=32mil KD1=4.5 DLEV=0 WD1=8mil + XW=-2mil KD2=4.5 NL=2 SP12=5mil $ ANALYSIS / PRINTS .TRAN .1NS 100NS .GRAPH IN1=V(STIM1) IN2=V(STIM2) VOUT1=V(TLOUT1) + VOUT2=V(TLOUT2) .GRAPH VOUT3=V(TLOUT3) VOUT4=V(TLOUT4) .END

zo = 75

5.5 v

zo = 75

14 HSPICE® Signal Integrity User Guide

X-2005.09

1: Introduction

Simulating Circuits with Signetics Drivers

Figure 12 Connecting I/O Chips with Transmission Lines

Here’s an netlist example of how I/O chips connect with transmission lInes:

* This examle connects I/O chips with transmission lines .OPTION SEARCH='$installdir/parts/signet' .OPTION POST=2 TNOM=27 NOMOD LIST METHOD=GEAR .TEMP 27 $ DEFINE PARAMETER VALUES .PARAM LV=0 HV=3 TD1=10n TR1=3n TF1=3n TPW=20n + TPER=100n TD2=20n TR2=2n TF2=2n LNGTH=101.6m $ POWER SUPPLY VCC VCC 0 DC 5.5 $ INPUT SOURCES VIN1 STIM1 0 PULSE LV HV TD1 TR1 TF1 TPW TPER VIN2 STIM2 0 PULSE LV HV TD2 TR2 TF2 TPW TPER $ FIRST STAGE: DRIVER WITH TLINE X1ST_TOP STIM1 OUTPIN1 VCC GND IO_CHIP PIN_IN=2.6n + PIN_OUT=4.6n X1ST_DN STIM2 OUTPIN2 VCC GND IO_CHIP PIN_IN=2.9n + PIN_OUT=5.6n U_1ST OUTPIN1 OUTPIN2 GND TLOUT1 TLOUT2 GND USTRIP L=LNGTH $ SECOND STAGE: RECEIVER WITH TLINE X2ST_TOP TLOUT1 OUTPIN3 VCC GND IO_CHIP PIN_IN=4.0n + PIN_OUT=2.5n X2ST_DN TLOUT2 OUTPIN4 VCC GND IO_CHIP PIN_IN=3.6n + PIN_OUT=5.1n U_2ST OUTPIN3 OUTPIN4 GND TLOUT3 TLOUT4 GND USTRIP L=LNGTH $ TERMINATING RESISTORS R1 TLOUT3 GND 75 R2 TLOUT4 GND 75

HSPICE® Signal Integrity User Guide 15 X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

$ IO CHIP MODEL - SIGNETICS .SUBCKT IO_CHIP IN OUT VCC XGND PIN_VCC=7n PIN_GND=1.8n X1 IN1 INVOUT VCC1 XGND1 ACTINPUT X2 INVOUT OUT1 VCC1 XGND1 AC109EQ *Package Inductance LIN_PIN IN IN1 PIN_IN LOUT_PIN OUT1 OUT PIN_OUT LVCC VCC VCC1 PIN_VCC LGND XGND1 XGND PIN_GND .ENDS $ TLINE MODEL - 2 SIGNAL CONDUCTORS WITH GND $ PLANE .MODEL USTRIP U LEVEL=3 ELEV=1 PLEV=1 + TH1=1.3mil HT1=10mil TS=32mil KD1=4.5 DLEV=0 WD1=8mil + XW=-2mil KD2=4.5 NL=2 SP12=5mil $ ANALYSIS / PRINTS .TRAN .1NS 100NS .GRAPH IN1=V(STIM1) IN2=V(STIM2) VOUT1=V(TLOUT1) + VOUT2=V(TLOUT2) .GRAPH VOUT3=V(TLOUT3) VOUT4=V(TLOUT4) .END

Simulating Circuits with Xilinx FPGAs

Synopsys and Xilinx maintain a library of HSPICE device models and transistor-level subcircuits for the Xilinx 3000 and 4000 series Field Programmable Gate Arrays (FPGAs). These subcircuits model the input and output buffer.

The following simulations use the Xilinx input/output buffer (xil_iob.inc) to simulate ground-bounce effects for the 1.08µm process at room temperature and at nominal model conditions. In the IOB and IOB4 subcircuits, y ou can set parameters to specify:

■

Local temperature.

■

Fast, slow, or typical speed.

■

1.2µ or 1.08µ technology.

You can use these choices to perform a variety of simulations to measure:

■

Ground bounce, as a function of package, temperature, part speed, and technology.

■

Coupled noise, both on-chip and chip-to-chip.

16 HSPICE® Signal Integrity User Guide

X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

■

Full transmission line effects at the package level and the printed circuit board level.

■

Peak current and instantaneous power consumption for power supply bus considerations and chip capacitor placement.

Syntax for IOB (xil_iob) and IOB4 (xil_iob4)

* EXAMPLE OF CALL FOR 1.2U PART: * X1 I O PAD TS FAST PPUB TTL VDD GND XIL_IOB *+ XIL_SIG=0 XIL_DTEMP=0 XIL_SHRINK=0 * EXAMPLE OF CALL FOR 1.08U PART: * X1 I O PAD TS FAST PPUB TTL VDD GND XIL_IOB *+ XIL_SIG=0 XIL_DTEMP=0 XIL_SHRINK=1

Nodes Description

I (IOB only) output of the TTL/CMOS receiver O (IOB only) input pad driver stage I1 (IOB4 only) input data 1 I2 (IOB4 only) input data 2 DRIV_IN (IOB4 only) PAD bonding pad connection TS three-state control input (5 V disables) FAST slew rate control (5 V fast) PPUB (IOB only) pad pull-up enable (0 V enables) PUP (IOB4 only) pad pull-up enable (0 V enables) PDOWN (IOB4 only) pad pull-up enable (5 V enables) TTL (IOB only) CMOS/TTL input threshold (5 V selects TTL) VDD 5-volt supply GND ground

HSPICE® Signal Integrity User Guide 17 X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

Nodes Description

XIL_SIG model distribution: (default 0)

XIL_DTEMP Buffer temperature difference from ambient. The

XIL_SHRINK Old or new part; (default is new):

All grounds and supplies are common to the external nodes for the g round and VDD. You can redefine grounds to add package models.

-3==> slow 0==> typical +3==> fast

default = 0 degrees if ambient is 25 degrees, and if the buffer is 10 degree s hotter than XIL_DTEMP=10.

0==>old 1==>new

Ground-Bounce Simulation

Ground-bounce simulation duplicates the Xilinx internal measurements methods. It simultaneously toggles 8 to 32 outputs. The simulation loads each output with a 56 pf capacitance. Simulation also uses an 84-pin package mode and an output buffer held at chip ground to measure the internal ground bounce.

Figure 13 Ground Bounce Simulation

< <

84plcc

pkg

18 HSPICE® Signal Integrity User Guide

X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

HSPICE or HSPICE RF adjusts the simulation model for the oscilloscope recordings so you can use it for the two-bond wire ground. For example, the following netlist simulates ground bounce:

qabounce.sp test of xilinx i/o buffers .OPTION SEARCH='$installdir/parts/xilinx' .op .option post list .tran 1ns 50ns sweep gates 8 32 4 .measure bounce max v(out1x) *.tran .1ns 7ns .param gates=8 .print v(out1x) v(out8x) i(vdd) power $.param xil_dtemp=-65 $ -40 degrees c $ (65 degrees from +25 degrees) vdd vdd gnd 5.25 vgnd return gnd 0 upower1 vdd return iob1vdd iob1gnd pcb_power + L=600mil * local power supply capacitors xc1a iob1vdd iob1gnd cap_mod cval=.1u xc1b iob1vdd iob1gnd cap_mod cval=.1u xc1c iob1vdd iob1gnd cap_mod cval=1u xgnd_b iob1vdd iob1gnd out8x out1x xil_gnd_test xcout8x out8x iob1gnd cap_mod m=gates xcout1x out1x iob1gnd cap_mod m=1 .model pcb_power u LEVEL=3 elev=1 plev=1 nl=1 llev=1 + th=1.3mil ht=10mil kd=4.5 dlev=1 wd=500mil xw=-2mil .macro cap_mod node1 node2 cval=56p Lr1 node1 node1x L=2nh R=0.05 cap node1x node2x c=cval Lr2 node2x node2 L=2nh R=0.05 .eom .macro xil_gnd_test vdd gnd outx outref + gates=8 * example of 8 iobuffers simultaneously switching * through approx. 4nh lead inductance * 1 iob is active low for ground bounce measurements vout drive chipgnd pwl 0ns 5v, 10ns 5v, 10.5ns 0v, $+ 20ns 0v, 20.5ns 5v, 40ns 5v R x8 I8 drive PAD8x TS FAST PPUB TTL chipvdd chipgnd + xil_iob xil_sig=0 xil_dtemp=0 xil_shrink=1 M=gates x1 I1 gnd PAD1x TS FAST PPUB TTL chipvdd chipgnd + xil_iob xil_sig=0 xil_dtemp=0 xil_shrink=1 m=1 *Control Settings rts ts chipgnd 1 rfast fast chipvdd 1 rppub ppub chipgnd 1

HSPICE® Signal Integrity User Guide 19 X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

rttl ttl chipvdd 1 * pad model plcc84 rough estimates lvdd vdd chipvdd L=3.0nh r=.02 lgnd gnd chipgnd L=3.0nh r=.02 lout8x outx pad8x L='5n/gates' r='0.05/gates' lout1x outref pad1x L=5nh r=0.05 c_vdd_gnd chipvdd chipgnd 100n .eom .end

Figure 14 Results of Ground Bounce Simulation

Coupled Line Noise

This example uses coupled noise to separate IOB parts. The output of one part drives the input of the other part through 0.6 inches of PCB. This example also monitors an adjacent quiet line.

20 HSPICE® Signal Integrity User Guide

X-2005.09

Figure 15 Coupled Noise Simulation

1: Introduction

Simulating Circuits with Xilinx FPGAs

Here’s an example netlist for coupled noise simulation:

Input File, for qa8.sp test of xilinx 0.8u i/o buffers .OPTION SEARCH='$installdir/parts/xilinx' .op .option nomod post=2 *.tran .1ns 5ns sweep xil_sig -3 3 3 .tran .1ns 15ns .print v(out1x) v(out3x) i(vdd) v(irec) vdd vdd gnd 5 vgnd return gnd 0 upower1 vdd return iob1vdd iob1gnd pcb_power L=600mil upower2 vdd return iob2vdd iob2gnd pcb_power L=600mil x4io iob1vdd iob1gnd out3x out1x outrec irec xil_iob4 cout3x out3x iob1gnd 9pf u1x out1x outrec iob1gnd i_o_in i_o_out iob2gnd pcb_top + L=2000mil xrec iob2vdd iob2gnd i_o_in i_o_out xil_rec .ic i_o_out 0v .model pcb_top u LEVEL=3 elev=1 plev=1 nl=2 llev=1 + th=1.3mil ht=10mil sp=5mil kd=4.5 dlev=1 wd=8mil xw=-2mil .model pcb_power u LEVEL=3 elev=1 plev=1 nl=1 llev=1 + th=1.3mil ht=10mil kd=4.5 dlev=1 wd=500mil xw=-2mil .macro xil_rec vdd gnd tri1 tri2 * example of 2 iobuffers in tristate xtri1 Irec O pad_tri1 TSrec FAST PPUB TTL + chipvdd chipgnd xil_iob xil_sig=0 xil_dtemp=0 xil_shrink=1

HSPICE® Signal Integrity User Guide 21 X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

+ m=1 xtri2 Irec O pad_tri2 TSrec FAST PPUB TTL + chipvdd chipgnd xil_iob xil_sig=0 xil_dtemp=0 + xil_shrink=1 m=1 *Control Setting rin_output O chipgnd 1 rtsrec tsrec chipvdd 1 rfast fast chipvdd 1 rppub ppub chipgnd 1 rttl ttl chipvdd 1 * pad model plcc84 rough estimates lvdd vdd chipvdd L=1nh r=.01 lgnd gnd chipgnd L=1nh r=.01 ltri1 tri1 pad_tri1 L=3nh r=0.01 ltri2 tri2 pad_tri2 L=3nh r=.01 c_vdd_gnd chipvdd chipgnd 100n .eom .macro xil_iob4 vdd gnd out3x out1x outrec Irec * example of 4 iobuffers simultaneously switching * through approx. 3nh lead inductance * 1 iob is a receiver (tristate) vout O chipgnd pwl 0ns 0v, 1ns 0v, 1.25ns 4v, 7ns 4v, + 7.25ns 0v, 12ns 0v R x3 I3 O PAD3x TS FAST PPUB TTL chipvdd chipgnd xil_iob + xil_sig=0 xil_dtemp=0 xil_shrink=1 m=3 x1 I1 O PAD1x TS FAST PPUB TTL chipvdd chipgnd xil_iob + xil_sig=0 xil_dtemp=0 xil_shrink=1 m=1 xrec Irec O PADrec TSrec FAST PPUB TTL chipvdd chipgnd xil_iob + xil_sig=0 xil_dtemp=0 xil_shrink=1 m=1 * control settings rts ts chipgnd 1 rtsrec tsrec chipvdd 1 rfast fast chipvdd 1 rppub ppub chipgnd 1 rttl ttl chipvdd 1 * pad model plcc84 rough estimates lvdd vdd chipvdd L=1nh r=.01 lgnd gnd chipgnd L=1nh r=.01 lout3x out3x pad3x L=1nh r=.0033 lout1x out1x pad1x L=4nh r=0.01 loutrec outrec padrec L=4nh r=.01 c_vdd_gnd chipvdd chipgnd 100n .eom .end

22 HSPICE® Signal Integrity User Guide

X-2005.09

Figure 16 Results of Coupled Noise Simulation

1: Introduction

Simulating Circuits with Xilinx FPGAs

Far End Driven line

Near End Driven line

Near and far end quite line

The I/O block model description:

* INPUT/OUTPUT BLOCK MODEL * PINS: * I OUTPUT OF THE TTL/CMOS INPUT RECEIVER. * O INPUT TO THE PAD DRIVER STAGE. * PAD BONDING PAD CONNECTION. * TS THREE-STATE CONTROL INPUT. HIGH LEVEL * DISABLES PAD DRIVER. * FAST SLEW RATE CONTROL. HIGH LEVEL SELECTS FAST SLEW RATE. * PPUB PAD PULLL-UP ENABLE. ACTIVE LOW. * TTL CMOS/TTL INPUT THRESHOLD SELECT. HIGH SELECTS TTL. * VDD POSITIVE SUPPLY CONNECTION FOR INTERNAL CIRCUITRY. * ALL SIGNALS ABOVE ARE REFERENCED TO NODE 0. * THIS MODEL CAUSES SOME DC CURRENT TO FLOW * INTO NODE 0, WHICH IS AN ARTIFACT OF THE MODEL. * GND CIRCUIT GROUND

The buffer module description:

* THIS SUBCIRCUIT MODELS THE INTERFACE BETWEEN XILINX * 3000 SERIES PARTS AND THE BONDING PAD. IT IS NOT * USEFUL FOR PREDICTING DELAY TIMES FROM THE OUTSIDE

HSPICE® Signal Integrity User Guide 23 X-2005.09

1: Introduction

Simulating Circuits with Xilinx FPGAs

* WORLD TO INTERNAL LOGIC IN THE XILINX CHIP. RATHER, * IT CAN BE USED TO PREDICT THE SHAPE OF WAVEFORMS * GENERATED AT THE BONDING PAD AS WELL AS THE RESPONSE * OF THE INPUT RECEIVERS TO APPLIED WAVEFORMS. * THIS MODEL IS INTENDED FOR USE BY SYSTEM DESIGNERS * WHO ARE CONCERNED ABOUT TRANSMISSION EFFECTS IN * CIRCUIT BOARDS CONTAINING XILINX 3000 SERIES PARTS. * THE PIN CAPACITANCE AND BONDING WIRE INDUCTANCE, * RESISTANCE ARE NOT CONTAINED IN THIS MODEL. THESE * ARE A FUNCTION OF THE CHOSEN PACKAGE AND MUST BE * INCLUDED EXPLICITLY IN A CIRCUIT BUILT WITH THIS * SUBCIRCUIT. * NON-IDEALITIES SUCH AS GROUND BOUNCE ARE ALSO A * FUNCTION OF THE SPECIFIC CONFIGURATION OF THE * XILINX PART, SUCH AS THE NUMBER OF DRIVERS WHICH * SHARE POWER PINS SWITCHING SIMULTANEOUSLY. ANY * SIMULATION TO EXAMINE THESE EFFECTS MUST ADDRESS * THE CONFIGURATION-SPECIFIC ASPECTS OF THE DESIGN. * .SUBCKT XIL_IOB I O PAD_IO TS FAST PPUB TTL VDD GND + XIL_SIG=0 XIL_DTEMP=0 XIL_SHRINK=1 .prot FREELIB ;]= $.[;qW.261DW3Eu0 VO\;:n[ $.[;qW.2’4%S+%X;:0[(3’1:67*8-:1:\[ kp39H2J9#Yo%XpVY#O!rDI$UqhmE%:\7%(3e%:\7\5O)1-5i# ; .ENDS XIL_IOB

24 HSPICE® Signal Integrity User Guide

X-2005.09

Describes S parameter and SP modeling as well as other topics related to the S element

You can use the S element to describe a multi-terminal network in AC, DC and TRAN circuit analyses within either Synopsys HSPICE or HSPICE RF. This chapter describes S parameter and SP modeling as well as other topics related to the S element. For more information about using the S element (S parameter) for mixed-mode analysis, see the HSPICE Simulation and Analysis User Guide.

S Parameter Model

2S Parameter Modeling Using the S Element

You can use small-signal parameters at the network terminals to characterize linear or non-linear networks that have sufficiently small signals. After you set the parameters, you can simulate the block in any external circuit. S parameters are widely used to characterize a linear network especially among designers of high-frequency circuits.

S parameters (S) in multi-port networks are defined as follows:

bSa⋅=

HSPICE® Signal Integrity User Guide 25 X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

In the preceding equation, a is an incident wave factor, and b is a reflected wave vector, defined as follows:

12⁄

vf⋅ Z

vb⋅ Z

12⁄

if⋅==

ib⋅==

The preceding equations use the following definitions:

■

vf is the forward voltage vector.

■

vb is the backward voltage vector.

■

ir is the forward current vector.

■

ib is the backward current vector.

■

Zr is the characteristic impedance matrix of the reference system.

■

Yr is the characteristic admittance matrix.

■

Zr and Yr satisfy the following relationship:

1–

The S parameters are frequency-dependent. When all ports are terminated with impedance matching, the forward w av e is z ero . This is because there is no reflection if the ports have no voltage/current source.

Using the Scattering Parameter Element

The S (scattering) Element gives you a convenient way to describe a multiterminal network. You can use the S element in conjunction with the generic frequency-domain model (.MODEL SP), or data files that describe frequency- varying behavior of a network, and provide discrete frequency-dependent data such as a Touchstone file and CITIfile (Common Instrumentation Transfer and Interchange file).

The S element supports DC, AC, and TRAN analyses, and Y (admittance) parameters. See the HSPICE Simulation and Analysis User Guide for more information.

26 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

In particular, the S parameter in the S element represents the generalized scattering parameter (S) for a multi-terminal network, which is defined as:

ref

⋅=

inc

Where:

■

Lower-case symbols denote vectors.

■

Upper-case symbols denote matrices.

■

is the incident voltage wave vector.

inc

■

is the reflected voltage wave vector (see Figure 17 on page 32).

ref

The S parameter and the Y parameter satisfy the following relationship:

YYrsIS–()IS+()1–Y

where Yr is the characteristic admittance matrix of the reference system. The following formula relates Yr to the Zr characteristic impedance matrix:

1–

YrsY

===

Yr'ZrsZ

Similarly, you can convert the Y parameter to the S parameter as follows:

SIZrsYZ

–()IZ

+ YZ

()

1–

S Element Syntax

Use the following S element syntax to show the connections within a circuit:

27 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

nd1 nd2...ndN Nodes of an S element (see Figure 17). Three kinds of

definitions are present:

• With no reference node ndRef, the default reference node in this situation is GND . Each node ndi (i=1~N) and GND construct one of the N ports of the S element.

• With one reference node, ndRef is defined. Each node ndi (i=1~N) and the ndRef construct one of the N ports of the S element.

• With an N reference node , each port has its own reference node. You can write the node definition in a clearer way as:

nd1+ nd1- nd2+ nd2- ... ndN+ ndN-

Each pair of the nodes (ndi+ and ndi-, i=1~N) constructs one of the N ports of the S element.

ndRef Reference node. MNAME Name of the S model. FQMODEL Frequency beha vior of the parameters ..MODEL statement of

sp type, which defines the frequency-dependent matrices array.

TYPE Parameter type:

S: (scattering) (default) Y: (admittance) Z: (impedance)

Zo Characteristic impedance value for the reference line

(frequency-independent). For multiple terminals (N>1), HSPICE or HSPICE RF assumes that the characteristic impedance matrix of the reference lines is diagonal, and that you set diagonal values to Zo. To specify more general types

of reference lines, use Zof. Default=50 .

Ω

28 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

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 do not set this value, the reciprocal v alue of risetime value is taken. (See.OPTION RISETIME in the HSPICE Command Reference for more information.)

• If you set a frequency that is smaller than the reciprocal value of the transient, then transient analysis performs circular convolution, and uses the reciprocal value of FBASE as its base period.

FMAX Maximum frequency use in transient analysis. Used as the

maximum frequency point for Inverse Fast Fourier Transformation (IFFT).

PRECFAC In almost all cases, you do not need to spe cify a value f or this

parameter. This parameter specifies the precondition factor keyword used for the precondition process of the S parameter. A precondition is used to avoid an infinite admittance matrix. The default is 0.75, which is good for most cases.

DELAYHANDLE Delay handler for transmission-line type parameters. Set

DELAYHANDLE to ON (or 1) to turn on the delay handle; set DELAYHANDLE to OFF (or 0) to turn off the delay handle

(default).

DELAYFREQ Delay frequency for transmission-line type parameters. The

default is FMAX. If the DELAYHANDLE is set to OFF, but DELAYFREQ is nonzero, HSPICE still simulates the S element in delay mode.

INTERPOLATION The interpolation method:

• STEP: piecewise step

• SPLINE: b-spline curve fit

• LINEAR: piecewise linear (default)

29 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

INTDATTYP Data type for the linear interpolation of the complex data.

• RI: real-imaginary based interpolation

• DBA: dB-angle based interpolation

• MA: magnitude-angle based interpolation (default)

HIGHPASS Method to extrapolate higher frequency points.

• 0: cut off

• 1: use highest frequency point

• 2: perform linear extrapolation using the highest 2 points

• 3: apply the window function to gradually approach the cut-off level (default)

LOWPASS Method to extrapolate lower frequency points.

• 0: cut off

• 1: use the magnitude of the lowest point

• 2: perform linear extrapolation using the magnitude of the lowest two points

MIXEDMODE Set to 1 if the parameters are represented in the mixed

mode.

DATATYPE A string used to determine the order of the indices of the

mixed-signal incident or reflected vector. The string must be an array of a letter and a number (Xn) where:

• X = D to indicate a differential term

= C to indicate a common term = S to indicate a single (grounded) term

• n = the port number

30 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

NOISE

DTEMP

Activates thermal noise.

1: element generates thermal noise

•

0 (default): element is considered noiseless

Temperature difference between the element and the circuit, expressed in °C. The default is 0.0.

Element temperature is calculated as:

T = Element temperature (°K)

= 273.15 (°K) + circuit temperature (°C)

+ DTEMP (°C)

Where circuit temperature is specified using either the

.TEMP statement, or by sweeping the global TEMP variab le

.DC, .AC, or .TRAN statements.

When a circuit temperature is set by defaults to 25 °C unless you use raises the default to 27 °C.

.TEMP statement or TEMP variable is not used, the

.OPTION TNOM, which

.OPTION SPICE, which

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.

31 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Figure 17 Terminal Node Notation

nd1

(+) [v]1

[vinc]1

[vref]1

. . .

[i]1

N+1 terminal system

(-)

ndR

(reference node)

. . .

[vinc]N

[i]N

[vref]N

ndN

(+) [v]N

S Model Syntax

Use the following syntax to describe specific S models:

Parameter Description

Smodel_name Name of the S model. S Specifies that the model type is an S model. N S model dimension, which is equal to the terminal number of an

S element and excludes the reference node.

32 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

FQMODEL Frequency behavior of the S,Y, or Z parameters. .MODEL

statement of sp type, which defines the frequency-dependent matrices array.

TSTONEFILE Name of a Touchstone file. Data contains frequency-dependent

array of matrixes. Touchstone files must follow the .s#p file extension rule, where # represents the dimension of the network.

For details, see Touchstone EIA/IBIS Open Forum (http://www.eda.org).

CITIFILE Name of the CITIfile , which is a data file that contains frequency-

dependent data. For details, see Using Instruments with ADS by Agilent

Technologies (http://www.agilent.com).

File Format Specification by the

TYPE Parameter type:

S: (scattering) (default) Y: (admittance) Z: (impedance)

Zo Characteristic impedance value of the ref erence line (frequency-

independent). For multi-terminal lines (N>1), HSPICE assumes that the characteristic impedance matrix of the reference lines are diagonal, and their diagonal values are set to Zo. You can also set a vector value f or non-unif orm diagonal values. Use Zof to specify more general types of a reference-line system. The default is 50.

FBASE Base frequency used for transient analysis. HSPICE uses this

value as the base frequency point for Fast Inverse Fourier Transformation (IFFT).

• If FBASE is not set, HSPICE uses a reciprocal of the transient period as the base frequency.

• If FBASE is set smaller than the reciprocal value of transient period, transient analysis performs circular convolution by using the reciprocal value of FBASE as a base period.

FMAX Maximum frequency for transient analysis. Used as the

maximum frequency point for Inverse Fast Fourier Transform (IFFT).

33 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

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 In almost all cases, you do not need to specify a value for this

parameter. This parameter specifies the precondition factor keyword used f or the precondition process of the S parameter . A precondition is used to avoid an infinite admittance matrix. The default is 0.75, which is good for most cases.

DELAYHANDLE Delay handler for transmission-line type parameters.

• 1 or ON activates the delay handler.

• 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. The

default is FMAX. If the DELAYHANDLE is set to OFF, but DELAYFREQ is nonzero, HSPICE still sim ulates the S element in delay mode.

MIXEDMODE Set to 1 if the parameters are represented in the mixed mode.

34 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Paramete r Model

Parameter Description

DATATYPE A string used to determine the order of the indices of the mixed-

signal incident or reflected vector . The string must be an arra y of a letter and a number (Xn) where:

• X = D to indicate a differential term

= C to indicate a common term = S to indicate a single (grounded) term

• n = the port number

XLINELENGTH 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.

S Element Data File Model Examples

The S model statement samples shown in Example 1 and Example 2 generate the same results.

Example 1 S Model Statement Code Sample

s1 n1 n2 n3 n_ref mname=smodel .model smodel s n=3 fqmodel=sfqmodel zo=50 fbase=25e6 fmax=1e9 s1 n1 n2 n3 n_ref fqmodel=sfqmodel zo=50 fbase=25e6 fmax=1e9

In Example 2, the S model statement has the characteristic impedance equal 100 instead of the 50 as defined in smodel. The impedance changes because the parameters defined in the S element statement have higher priority than the parameters defined in the S Model statement.

Example 2 S Model Statement with Character Impedance of 100

s1 n1 n2 n3 n_ref mname=smodel zo=100 .model smodel s n=3 fqmodel=sfqmodel zo=50 fbase=25e6 fmax=1e9

HSPICE® Signal Integrity User Guide 35 X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

In Example 3, fqmodel, tstonefile, and citifile are all declared in

smodel. HSPICE accepts tstonefile, ignores both fqmodel and citifile, and issues a warning message. It is illegal to define a tstonefile and CITIfile smodel in the same statement. This prevents

conflicts in the frequency-varying behavior description of the network. From the

tstonefile file extension .s3p, you can tell that the network has three ports. Example 3 S Model Statement with fqmodel, tstonefile, and citifile

s1 n1 n2 n3 n_ref mname=smodel .model smodel s tstonefile=exp1.s3p fqmodel=sfqmodel

citifile=exp1.citi0

In Example 4, fqmodel is declared both in the S element statement and the S Model statement. Each statement refers to a different fqmodel, which is not allowed.

Example 4 S Model Statement with fqmodel declared in both the S element

statement and the S Model statement

s1 n1 n2 n3 n_ref mname=smodel fqmodel=sfqmodel_1 .model smodel s n=3 fqmodel=sfqmodel_2

A generic S parameter statement is shown in Example 5.

Example 5 S Parameter Example

**S-parameter example .option sim_mode=hspice .OPTION post=2 .probe v(n2) V1 n1 0 ac=1v PULSE 0v 5v 5n 0.5n 0.5n 25n .ac lin 500 1Hz 30MegHz .tran 0.1ns 10ns * reference node is set S1 n1 n2 0 mname=s_model * S parameter .model s_model S TSTONEFILE = ss_ts.s2p Rt1 n2 0 50 .end

In Example 6, the option line and noise parameters of a Touchstone file are shown.

36 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Paramete r Model

Example 6 Touchstone Example

! ! touchstone file example ! # Hz S MA R 50.0000

0.00000 0.637187 180.000 0.355136 0.00000

0.355136 0.00000 0.637187 180.000

......

! # HZ S DB R 50.0000 ! 0.00000 -3.91466 180.000 -8.99211 0.00000 ! -8.99211 0.00000 -3.91466 180.000

! ......

! !# Hz S RI R 50.0000 ! 0.00000 -0.637187 0.00000 0.355136 0.00000 ! 0.355136 0.00000 -0.637187 0.00000

! ......

! ! 2-port noise parameter ! frequency[Hz] Nfmin[dB] GammaOpt(M) GammaOpt(P) RN/Zo

0.0000 0.29166 0.98916 180.00 0.11055E-03

0.52632E+08 6.2395 0.59071 -163.50 0.32868

0.10526E+09 7.7898 0.44537 175.26 0.56586

! ......

! end of file

In Example 7, a S parameter statement and its referenced CITIfile are shown.

Example 7 S Parameter with CITIfile

**S-parameter .option sim_mode=hspice .OPTION post=2 .probe v(n2) V1 n1 0 ac=1v PULSE 0v 5v 5n 0.5n 0.5n 25n .ac lin 500 1Hz 30MegHz .tran 0.1ns 10ns * reference node is set *S1 n1 n2 0 mname=s_model * use default reference node S1 n1 n2 mname=s_model * S parameter .model s_model S CITIFILE = ss_citi.citi Zo=50 Rt1 n2 0 50 .end

# # citifile example "ss_citi.citi" #

HSPICE® Signal Integrity User Guide 37 X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

# CITIFILE A.01.00 NAME test VAR FREQ MAG 1 DATA S[1,1] DB DATA S[1,2] DB DATA S[2,1] DB DATA S[2,2] DB SEG_LIST_BEGIN SEG 1000 1000 1 SEG_LIST_END # BEGIN #0.333333333 0.0

-9.54242510308 0.0 END BEGIN #0.666666667 0.0

-3.52182518107 0.0 END BEGIN #0.666666667 0.0

-3.52182518107 0.0 END BEGIN #0.333333333 0.0

-9.54242510308 0.0 END # end of file

S Element Noise Model

This section describes how the S element supports two-port noise parameters and multiport passive noise models.

Two-Port Noise Parameter Support in Touchstone Files

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.

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).

38 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Paramete r Model

Input Interface

The frequency-dependent two-port noise parameters are provided in a network description block of a Touchstone data file following the S parameter data block.

The noise parameter data is typically organized by using the following syntax:

frequency[Hz] Nfmin[dB] GammaOpt(M) GammaOpt(P) RN/Zo { ...data... }

Where:

■

frequency = frequency in units

■

Nfmin[dB] = minimum noise figure (in dB)

■

GammaOpt(M) = magnitude of reflection coefficient needed to realize Fmin

■

GammaOpt(P) = phase (in degrees) of reflection coefficient needed to realize Fmin

■

RN/Zo = normalized noise resistance

■

! = indicates a comment line

For example:

! 2-port noise parameter ! frequency[Hz] Nfmin[dB] GammaOpt(M) GammaOpt(P) RN/Zo

0.0000 0.29166 0.98916 180.00 0.11055E-03

0.52632E+08 6.2395 0.59071 -163.50 0.32868

0.10526E+09 7.7898 0.44537 175.26 0.56586

Both GammaOpt and RN/Zo values are normalized with respect to the characteristic impedance, Zo, specified in the header of the Touchstone data file. HSPICE reads this raw data and converts it to a coefficient of the noisecurrent correlation matrix. This matrix can be stamped into an HSPICE noise analysis as two correlated noise current sources: j1 and j2, as shown here:

2j1

∗

j1j

∗

The noise-current correlation matrix represents the frequency-dependent statistical relationship between two noise current sources, j

and j2, as

illustrated in the follo w ing figure.

HSPICE® Signal Integrity User Guide 39 X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Original System

Noisy System

S Element

j1 j2

Transformed System

Noiseless System

S Element

Output Interface

HSPICE creates a .lis output list file that shows the results of a noise analysis just as any other noisy elements. The format is as following:

**** s element squared noise voltages (sq v/hz) element 0:s1

N11 data

r(N11) data

N12 data

r(N12) data

N21 data

r(N21) data

N22 data

r(N22) data

total data

Where:

■

N11 = contribution of j1 to the output port

■

r(N11) = transimpedance of j1 to the output port

■

N12 = contribution of j1j2* to the output port

■

r(N12) = transimpedance of j1 to the output port

■

N21 = contribution of j2j1* to the output port

■

r(N21) = transimpedance of j2 to the output port

■

N22 = contribution of j2 to the output port

■

r(N22) = transimpedance of j2 to the output port

■

total = contribution of total noise voltage of the S element to the output port.

40 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

S Paramete r Model

Notifications and Limitations

Because Touchstone files currently provide only two-port noise parameters, this type of noise model only supports two-port S parameter noise analysis for both passive and active systems.

Multiport Noise Model for Passive Systems

Multiport passive and lossy circuits, such as transmission lines and package parasitics, can exhibit considerable thermal noise. The passive noise model is used to present such thermal noise for the S element representing such circuits. The S element passive noise model supports both normal and two-port noise analysis (.NOISE and .LIN noisecalc=1).

Input Interface

To trigger a passive multiport noise model, the NOISE and DTEMP keywords in an S element statement are used:

Sxxx n1...nN + ... + <NOISE=[1|0]> <DTEMP=value>

Parameter Description

NOISE Activates thermal noise.

1: element generates thermal noise

•

0 (default): element is considered noiseless

•

HSPICE® Signal Integrity User Guide 41 X-2005.09

2: S Parameter Modeling Using the S Element

S Parameter Model

Parameter Description

DTEMP Temperature diff erence between the element and the circuit, expressed in

°C. The default is 0.0. Element temperature is calculated as:

T = Element temperature (°K)

= 273.15 (°K) + circuit temperature (°C)

+ DTEMP (°C)

Where circuit temperature is specified using either the or by sweeping the global TEMP variable in statements.

When a temperature is set by you use

.TEMP statement or TEMP variable is not used, the circuit

.OPTION TNOM, which defaults to 25 °C unless

.OPTION SPICE, which raises the default to 27 °C.

.DC, .AC, or .TRAN

.TEMP statement,

When NOISE=1, HSPICE generates a N×N noise-current correlation matrix from the N×N S parameters according to Twiss' Theorem. The result can be stamped into an HSPICE noise analysis as N-correlated noise current sources: ji (i=1~N), as shown below:

∗

C 2kT Y Y

∗

+()

2j1

j1j

∗

… j

… j2j

1jN

∗ ∗

… ………

Nj1

∗

Nj2

∗

… j

Where

YYcIS–()IS+()

1–

The noise-current correlation matrix represents the frequency-dependent statistical relationship between N noise current sources, j

(i=1~N), shown in the

following figure.

42 HSPICE® Signal Integrity User Guide

X-2005.09

Port 2

Port 1

2: S Parameter Modeling Using the S Element

Original System Transformed System

...

Port i

Lossy Passive N-Port

Port j

Port N–1

Port N

Port 2

Port 1

Port i

Lossless Passive N-Port System

Port j

S Paramete r Model

Port N–1

N–1

Port N

Output Interface

HSPICE creates a .lis output list file that shows the results of a noise analysis just as any other noisy elements. The format is as following:

**** s element squared noise voltages (sq v/hz)

element 0:s1 N(i,j) data r(N(i,j)) data ... i,j = 1~N ... total data

Where:

■

N(i,j) = contribution of jijj* to the output port

■

r(N(i,j)) = transimpedance of ji to the output port

■

total = contribution of total noise voltage of the S element to the output port.

Notifications and Limitations

Because the S element can support two kinds of noise models, the priority is:

■

For multisport (N≠2) S elements, only passive noise models are considered in noise analysis. If NOISE=0, the system is considered as noiseless.

HSPICE® Signal Integrity User Guide 43 X-2005.09

2: S Parameter Modeling Using the S Element

Mixed-Mode S Parameters

■

For two-port S elements, if two-port noise parameters are provided in a Touchstone file, the noise model is generated from those two-port noise parameters. If two-port noise parameters are not provided and NOISE=1, then a passive noise model is triggered. Otherwise, the system is considered as noiseless.

Mixed-Mode S Parameters

Mixed-mode refers to a combination of Differential and Common mode characteristics in HSPICE linear network analysis by using the S element.

Figure 18 Node Indexing Convention

Sxxx n1 n2 n3 n4 [nref] mname=xxx

Line B

Line A

n2n1

n4n3

■

You can use mixed-mode S parameters only with a single pair of transmission lines (4 ports).

■

Nodes 1 and 3 are the ports for one end of the transmission-line pair.

■

Nodes 2 and 4 are the ports for the opposite end of the transmission-line pair.

Relating Voltage and Current Waves to Nodal Waves

The following figure and set of equations include common and diff erential mode voltage and current waves, relating them to nodal waves. Although you can apply mixed-mode data propagation to an arbitrary number of pairs of transmission lines, a single pair model is used here.

Figure 19 shows a schematic of symmetric coupled pair transmission lines commonly used for the differential data transfer system.

44 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Mixed-Mode S Parameters

Figure 19 Schematic of Symmetric Coupled-Pair Transmission Line

port 1

Line A

Line B

port 2

Solving the telegrapher’s equation, you can represent nodal voltage and current waves of the data transfer system as:

γ–ex

A1e

++ +=

γ–ex

A1e

γ–ex

------- e

A2e

------- e Z

γex

A3e

γex

A3e

– A4e

γex

------- e Z

γ–ox

–+=

–+–=

A4e

------- e Z

γox

γ–ex

------- e Z

------Z

γex

– e

++–=

------Z

γ–ox

------Z

γox

(1)

Where:

■

γe is the propagation constant for even mode waves.

■

γo is the propagation constant for odd mode waves.

■

Ζe is the characteristic impedance for even mode waves.

■

Ζo is the characteristic impedance for odd mode waves.

■

A1 and A3 represent phasor coefficients for the forw ard propagating modes .

■

A2 and A4 represent phasor coefficients for the backward propagating modes.

HSPICE® Signal Integrity User Guide 45 X-2005.09

2: S Parameter Modeling Using the S Element

Mixed-Mode S Parameters

Each voltage and current pair at each node represents a single propagating signal wav e referenced to the g round potential. This type of expression is called nodal wav e representation.

Characterizing Differential Data Transfer Systems

The following equations use differential and common mode waves to characterize differential data transf er systems. The diff erence of the nodal wav e defines the voltage and current of the differential wave:

dmv1v3

–≡

---i1i–

()≡

Common mode voltage and current are defined as:

---v1v3+()≡ 2

+≡

cmi1i3

Deriving a Simpler Set of Voltage and Current Pairs

In the following e xample , substituting equations 2 and 3 into equation 1 derives a simpler set of voltage and current pairs:



2A3e



γex–

γox–

A1e

A2e

γox–

A4e

γex

γ–ox

46 HSPICE® Signal Integrity User Guide

------- e Z



------- e





–=

γ–ex

------- e Z

------- e

–

γox

2 e

γex

X-2005.09

2: S Parameter Modeling Using the S Element

Mixed-Mode S Parameters

You can also relate characteristic impedances of each mode to the even and odd mode characteristic impedances:

≡

------ -

≡

Having defined a generalized parameter power wave in this example, you can now define differential normalized waves at port 1 and port 2:

dm1

≡

-----------------------------------------

dmZdm

≡ b

--------------------------------------

Zdmi

– i

x0=

dm2

≡

-----------------------------------------

dmZdm

≡

--------------------------------------

– i

Zdmi

xL=

(2)

xL=

Similarly, you can define common mode normalized waves as:

cm1

cmZcmicm

≡ a

---------------------------------------2Z

x0=

cm2

≡

----------------------------------------

Zcmi

xL=

– i

cm1

HSPICE® Signal Integrity User Guide 47 X-2005.09

cmZcm

≡ b

-------------------------------------

cm2

x0=

– i

cmZcm

≡

------------------------------------2Z

(3)

xL=

2: S Parameter Modeling Using the S Element

Mixed-Mode S Parameters

You can then specify S-parameters for mixed-mode waves as ratios of these waves:

dm1

dm2

cm1

cm2

mixed

dm1

dm2

cm1

cm2

mixed

=,=

SddS S

cdScc

(4)

Where:

■

Sdd is the differential-mode S parameter

■

Scc is the common-mode S parameter

■

Scd and Sdc represent the mode-conversion or cross-mode S parameters

Based on these definitions, you can linearly transform nodal wav e (standard) Sparameters and mixed mode S-parameters:

⋅⋅S

s dardtan

1–

mixed

(5)

The M transformation matrix is:

10 1– 0

01 0 1–

-------

10 1 0

(6)

01 0 1

Using the Mixed-Mode S Parameters (S Element)

The S element can recognize and parse the mixed-mode S parameters when the mixedmode=1 keyword is set. Any other keywords besides mixedmode and datatype remain the same. Use the f ollo wing syntax for a mixed-mode S parameter.

Sxxx p1+ <p1-> p2+ <p2-> p3+ <p3->...[n_ref] mname=Smodel .MODEL Smodel S ... [+ mixedmode=<0 | 1>] [+ datatype=XiYjZk...]

48 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Mixed-Mode S Parameters

The pn+ and pn- are the positive and negative terminals of the port n, respectively. If the port is in mixed mode (balanced) one, both positive and negative terminal names are required in series; if the port is single-ended, only one terminal name is required. The port numbers must be in increasing order corresponding to the S matrices notation.

Table 2 Mixed-Mode S Parameter Keywords

Parameter Description

mixedmode When mixedmode=1, the t the element knows that the S

parameters are defined in mixed mode. The default is 0 (standardmode)

datatype A string that determines the order of indices of the incident or

reflected vectors (a and b) in Equation 8. The string must be an array of pairs that consists of a letter and a number (for example, Xn), where X=

• D or d to indicate differential term

• C or c to indicate common term

• S, s, G or g to indicate single (grounded) term and n = port number.

The definition datatype = D1D2C1C2 is the default for a 2-balanced port network and specifies the nodal relationship of the following equation:

standard

= [a1+ a1- a2+ a2-]T <=> a

= [ad1 ad2 ac1 ac2]

mixed

Where:

■

a1+ is the incident wave goes into positive terminal of the port 1

■

a1- is the incident wave goes into negative terminal of the port 1

■

a2+ is the incident wave goes into positive terminal of the port 2

■

a2- is the incident wave goes into negative terminal of the port 2

You can also derive the nodal relationship of the reflection wave in the same way. Nodes are assigned from the given s-matrices to the S element in the order of a

standard

. For example, incident and reflected waves at the positive

terminal of the 1(a1+, b1+) port appear at the first node of the S element.

HSPICE® Signal Integrity User Guide 49 X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

The definition datatype = D1C1S2 specifies the nodal relationship of the following equation:

standard

= [a1+ a1- a2]T <=> a

= [ad1 ac1 as2]

mixed

The default of nodemap is nodemap=D1D2...DnC1C2...Cn, which is available for systems with mixed-mode (balanced) ports only.

Mixed-Mode S Parameter Netlist Examples

Example 8 Differential Transmission Line Pair

You can find an example netlist for a differential transmission line pair in the following directory:

$installdir/demo/hspice/sparam/mixedmode_s.sp

Example 9 Differential Amplifier

You can find an example netlist for a differential amplifier in the following directory:

$installdir/demo/hspice/sparam/diffamp_s.sp

Small-Signal Parameter Data-Table Model

The Small-Signal Parameter Data-Table Model (SP model) is a generic model that describes frequency-varying behavior.

SP Model Syntax

.MODEL name sp [N=val FSTART=val FSTOP=val NI=val + SPACING=val MATRIX=val VALTYPE=val INFINITY=matrixval + INTERPOLATION=val EXTRAPOLATION=val] [DATA=(npts ...)] + [DATAFILE=filename]

50 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

Note: Interpolation and extrapolation occur after the simulator internally

converts the Z and S parameter data to Y parameter data.

Parameter Specifies

name Model name. N Matrix dimension (number of signal terminals). Default is 1. If you

use a value other than the default, you must specify that value

before you set INFINITY and DATA. FSTART Starting frequency point for data. Default=0. FSTOP Final frequency point for data. Use this parameter only for the

LINEAR and LOG spacing formats. NI Number of frequency points per interval. Use this parameter only

for the DEC and OCT spacing formats. Default=10. SPACING Data sample spacing format:

• LIN (LINEAR): uniform spacing with frequency step of (FSTOP-FSTART)/(npts-1). The default.

• OCT: octav e variation with FSTART as the starting frequency , and NI points per octave. npts sets the final frequency.

• DEC: decade variation with FSTART as the starting frequency, and NI points per decade. npts sets the final frequency.

• LOG: logarithmic spacing. FSTART and FSTOP are the starting and final frequencies.

• POI: non-uniform spacing. Pairs data

• (NONUNIFORM) points with frequency points.

MATRIX Matrix (data point) format:

• SYMMETRIC: symmetric matrix. Specifies only lower-half triangle of a matrix (default).

• HERMITIAN: similar to SYMMETRIC; off-diagonal terms are complex-conjugates of each other.

• NONSYMMETRIC: non-symmetric (full) matrix.

HSPICE® Signal Integrity User Guide 51 X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

Parameter Specifies

VALTYPE Data type of matrix elements:

• REAL: real entry.

• CARTESIAN: complex number in real/imaginary format (default).

• POLAR: complex number in polar format. Specify angles in radians.

INFINITY Data point at infinity . Typically real-valued. This data format must

be consistent with MATRIX and VALTYPE specifications. npts does not count this point.

INTERPOLATION Interpolation scheme:

• STEP: piecewise step. This is the default.

• LINEAR: piecewise linear.

• SPLINE: b-spline curve fit.

EXTRAPOLATION Extrapolation scheme dur ing simulation:

• NONE: no extrapolation is allo wed. Simulation terminates if a required data point is outside of the specified range.

• STEP: uses the last boundary point. The default.

• LINEAR: linear extrapolation by using the last two boundary points.

If you specify the data point at infinity, then simulation does not

extrapolate and uses the infinity value. npts Number of data points. DC Data port at DC. Normally real-valued. This data f ormat must be

consistent with MATRIX and V ALTYPE specifications. npts does

not count this point. You must specify either the DC point or the

data point at frequency=0.

52 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

Parameter Specifies

DA TA Data points.

• Syntax for LIN spacing:

.MODEL name sp SPACING=LIN [N=dim] FSTART=f0

+ DF=f1 DATA=npts d1 d2 ...

• Syntax for OCT or DEC spacing:

.MODEL name sp SPACING=DEC or OCT [N=dim]

+ FSTART=f0 NI=n_per_intval DATA=npts d1 d2 ...

• Syntax for POI spacing:

.MODEL name sp SPACING=NONUNIFORM [N=dim]

+ DATA=npts f1 d1 f2 d2 ... DA TAFILE Data points in an external file. This file must contain only raw

numbers without any suffixes , comments or continuatio n letters.

The order of data must be the same as in the DATA statement.

This data file has no limitation on line length so you can enter a

large number of data points.

Examples

.MODEL fmod SP N=2 FSTOP=30MegHz + DATA = 2 * matrix at f=0 + 0.02 0.0 * Re(Y11) Im(Y11) + -0.02 0.0 0.02 0.0 * Im(Y21) Im(Y21) (= Y21) Re(Y22) Im(Y22) * matrix at f=30MHz + 0.02 0.0 * Re(Y11) Im(Y11) + -0.02 0.0 0.02 0.0 * Im(Y21) Im(Y21) (= Y21) Re(Y22) Im(Y22)

.MODEL fmod SP N=2 FSTOP=30MegHz MATRIX=NONSYMMETRIC + DATA = 2 * matrix at f=0 + 0.02 0.0 -0.02 0.0 * Re(Y11) Im(Y11) Re(Y12) Im(Y12) + -0.02 0.0 0.02 0.0 * Im(Y21) Im(Y21) Re(Y22) Im(Y22) * matrix at f=30MHz + 0.02 0.0 -0.02 0.0 * Re(Y11) Im(Y11) Re(Y12) Im(Y12) + -0.02 0.0 0.02 0.0

HSPICE® Signal Integrity User Guide 53 X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

* Im(Y21) Im(Y21) Re(Y22) Im(Y22)

.MODEL fmod SP N=2 SPACING=POI + DATA = 1 + 0.0 * first frequency point * matrix at f=0 + 0.02 0.0 * Re(Y11) Im(Y11) + -0.02 0.0 0.02 0.0 * Im(Y21) Im(Y21) (= Y21) Re(Y22) Im(Y22) + 30e+6 * second frequency point * matrix at f=30MHz + 0.02 0.0 * Re(Y11) Im(Y11) + -0.02 0.0 0.02 0.0 * Im(Y21) Im(Y21) (= Y21) Re(Y22) Im(Y22)

.MODEL fmod SP N=2 FSTOP=30MegHz VALTYPE=REAL + DATA = 2 * matrix at f=0 + 0.02 -0.02 * Y11 Y12 + -0.02 0.02 * Y21 Y22 * matrix at f=30MHz + 0.02 -0.02 * Y11 Y12 + -0.02 0.02 * Y21 Y22

**S-parameter example .option sim_mode=hspice .OPTION post=2 .probe v(n2) V1 n1 0 ac=1v PULSE 0v 5v 5n 0.5n 0.5n 25n .op .ac lin 500 1Hz 30MegHz .tran 0.1ns 10ns *S1 n1 n2 0 mname=s_model S1 n1 n2 0 mname=s_model .model s_model S fqmodel=fmod Zo=50 50 *.model s_model S fqmodel=fmod2 Zo=50 100 * S parameter for Zo=(50 50) .MODEL fmod SP N=2 FSTOP=30MegHz DATA = 1 + 0.333333333 0.0 0.666666667 0.0 0.333333333 0.0 * S parameter for Zo=(50 100) .MODEL fmod2 SP N=2 FSTOP=30MegHz MATRIX=NONSYMMETRIC

54 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

+ DATA = 1 + 0.5 0.0 0.5 0.0 + 1.0 0.0 0.0 0.0 Rt1 n2 0 50 .end

Example 10 Transmission Line Using Resistive Termination

Figure 20 illustrates a transmission line that uses a resistive termination, and Table 3 shows a corresponding input file listing. In this example, the two outputs from the resistor and S parameter modeling must match exactly.

Figure 20 Transmission Line with Resistive Termination

Four-conductor line

Ro, L, Go, C, Rs, Gd

Reference conductor

Table 3 Input File Listing

Header, options, and sources

Termination x1 o1 o2 o3 0 terminator Transmission

line (W Element)

*S-parameter x-line with a resistive positive

termination

.OPTION POST V1 i1 0 ac=1v

W1 i1 i2 i3 0 o1 o2 o3 0 RLGCMODEL=wrlgc N=3 + L=0.97 .MODEL wrlgc W MODELTYPE=RLGC N=3 + Lo = 2.78310e-07 + 8.75304e-08 3.29391e-07 + 3.65709e-08 1.15459e-07 3.38629e-07 + Co = 1.41113e-10 + -2.13558e-11 9.26469e-11 + -8.92852e-13 -1.77245e-11 8.72553e-11

HSPICE® Signal Integrity User Guide 55 X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

Frequency model definition

Resistor elements

Analysis .AC lin 500 0Hz 30MegHz

Equivalent S parameter element

.MODEL fmod sp N=3 FSTOP=30MegHz + DATA= 1 + -0.270166 0.0 + 0.322825 0.0 -0.41488 0.0 + 0.17811 0.0 0.322825 0.0 -0.270166 0.0

.SUBCKT terminator n1 n2 n3 ref

R1 n1 ref 75 R2 n2 ref 75 R3 n3 ref 75 R12 n1 n2 25 R23 n2 n3 25

.ends terminator

.DC v1 0v 5v 1v

.ALTER S parameter case .SUBCKT terminator n1 n2 n3 ref S1 n1 n2 n3 ref + FQMODEL=fmod .ENDS terminator .END

Example 11 Transmission Line Using Capacitive Network Termination

The transmission line example shown here uses capacitive network termination. The two outputs from the resistor and S parameter modeling in Example 10 differ slightly due to the linear frequency dependency relative to

56 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

the capacitor. To remove this difference, use the linear interpolation scheme in .MODEL.

Frequency model definition

.MODEL fmod sp N=3 FSTOP=30MegHz + DATA= 2 + 1.0 0.0 + 0.0 0.0 1.0 0.0 + 0.0 0.0 0.0 0.0 1.0 0.0 + 0.97409 -0.223096 + 0.00895303 0.0360171 0.964485 -0.25887 + -0.000651487 0.000242442 0.00895303 + 0.0360171 0.97409 -0.223096

Using capacitive elements

.SUBCKT terminator n1 n2 n3 ref

C1 n1 ref 10pF C2 n2 ref 10pF C3 n3 ref 10pF C12 n1 n2 2pF C23 n2 n3 2pF

.ENDS terminator

Example 12 Transmission Line Using S Parameter

Figure 21 and Table 4 show an example of a transmission line that uses the S parameter.

Figure 21 3-Conductor Transmission Line

3-conductor line

Ro, L, Go, C, Rs, Gd

HSPICE® Signal Integrity User Guide 57 X-2005.09

Reference conductor

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

Table 4 Input File Listing

Header, options, and sources

*S parameter ex3: modeling x-line by using + S parameter .OPTION POST vin in0 0 ac=1

Analysis .AC lin 100 0 1000meg

.DC vin 0 1v 0.2v

Transmission line W1 in1 in2 0 out1 out2 0 N=2 RLGCMODEL=m2 Termination R1 in0 in1 28

R2 in2 0 28 R3 out1 0 28 R4 out2 0 28

WElement RLGC model definition

.MODEL m2 W ModelType=RLGC, N=2 + Lo= 0.178e-6 0.0946e-7 0.178e-6 + Co= 0.23e-9 -0.277e-11 0.23e-9 + Ro= 0.97 0 0.97 + Go= 0 0 0 + Rs= 0.138e-3 0 0.138e-3 + Gd= 0.29e-10 0 0.29e-10

58 HSPICE® Signal Integrity User Guide

X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

Frequency model definition

Equivalent S parameter element

.MODEL SM2 sp N=4 FSTART=0 FSTOP=1e+09 + SPACING=LINEAR + DATA= 60 + 0.00386491 0 + 0 0 0.00386491 0 + 0.996135 0 0 0 0.00386491 0 + 0 0 0.996135 0 0 0 0.00386491 0 + -0.0492864 -0.15301 + 0.00188102 0.0063569 -0.0492864 + -0.15301 0.926223 -0.307306 0.000630484 + -0.00154619 0.0492864 -0.15301 + 0.000630484 -0.00154619 0.926223 + -0.307306 0.00188102 0.0063569 + -0.0492864 -0.15301 -0.175236 -0.241602 + 0.00597 0.0103297 -0.175236 -0.241602 + 0.761485 -0.546979 0.00093508 + -0.00508414 -0.175236 -0.241602 + 0.00093508 -0.00508414 0.761485 + -0.546979 0.00597 0.0103297 -0.175236 + -0.241602 +...

.SUBCKT terminator n1 n2 n3 ref

S1 n1 n2 n3 ref FQMODEL=SM2 .ENDS terminator .END

HSPICE® Signal Integrity User Guide 59 X-2005.09

2: S Parameter Modeling Using the S Element

Small-Signal Parameter Data-Table Model

60 HSPICE® Signal Integrity User Guide

X-2005.09

3Modeling Coupled Transmission Lines

Using the W Element

Describes how to use basic transmission line simulation equations and an optional method for computing the parameters of transmission line equations.

A transmission line is a passive element that connects any two conductors, at any distance apart. One conductor sends the input signal through the transmission line and the other conductor receives the output signal from the transmission line. The signal that transmits from one end of the pair to the other end is voltage between the conductors.

Examples of transmission lines include:

■

Power transmission lines

■

Telephone lines

■

Waveguides

■

Traces on printed circuit boards and multi-chip modules (MCMs)

■

Bonding wires in semiconductor IC packages

■

On-chip interconnections

This chapter describes the basic transmission line simulation equations. It explains how to use these equations as an input to the tr ansmission line model,

HSPICE® Signal Integrity User Guide 61 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Equations and Parameters

the W Element. (For more information about the W Element, see Dmitri Kuznetsov, “Optimal Transient Simulation of Transmission Lines,” IEEE Trans., Circuits Syst., vol.43, pp. 110-121, Feb., 1996.)

This chapter also shows you an optional method for computing the parameters of the transmission line equations using the field solver model.

The W Element is a versatile transmission line model that you can apply to efficiently and accurately simulate transmission lines, ranging from a simple lossless line to complex frequency-dependent lossy-coupled lines. Unlik e the U Element, the W Element can output accurate simulation results without finetuning optional parameters. For more information on U Elements, see Chapter

5, “Modeling Ideal and Lumped Transmission Lines.”

Transmission line simulation is challenging and time-consuming, because extracting transmission line parameters from physical geometry requires a significant effort. To minimize this effort, you can use a simple (but efficient and accurate) 2-D electromagnetic field solver, which calculates the electrical parameters of a transmission line system, based on its cross-section.

Equations and Parameters

Maxwell’s equations for the transverse electromagnetic (TEM) waves on multiconductor transmission lines, reduce to the telegrapher’s equations. The general form of the telegrapher’s equation in the frequency domain is:

∂

vzω,()– R ω() jωL ω()+[]izω,()=

z∂

∂

izω,()– G ω() jωC ω()+[]vzω,()=

z∂

The preceding equations use the following definitions:

■

Lower-case symbols denote vectors.

■

Upper-case symbols denote matrices.

■

v is the voltage vector across the lines.

■

i is the current vector along the lines.

For the TEM mode, the tr ansverse distribution of electromagnetic fields at any instant of time is identical to that for the static solution.

62 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Frequency-Dependent Matrices

From a static analysis, you can derive the four parameter matrices for multiconductor TEM transmission lines:

■

resistance matrix, R

■

inductance matrix, L

■

conductance matrix, G

■

capacitance matrix, C

The telegrapher’s equations, and the four parameter matrices from a static analysis, completely and accurately describe TEM lines.

Unfortunately, not all transmission lines support pure TEM waves; some multiconductor systems inherently produce longitudinal field components. In particular, waves propagating in either the presence of conductor losses or the absence of dielectric homogeneity (but not dielectric losses), must have longitudinal components.

However, if the transverse components of the fields are significantly larger than the longitudinal components, the telegrapher’s equations (and the four parameter matrices obtained from a static analysis) still provide a good approximation. This is known as a quasi-static approximation.

Multi-conductor systems in which this approximation is valid, are called quasiTEM lines. For typical micro-strip systems , the quasi-static approximation holds up to a few gigahertz.

Frequency-Dependent Matrices

The static (constant) L and C matrices are accurate for a wide range of frequencies. In contrast, the static (DC) R matrix applies to only a limited frequency range, mainly due to the skin eff ect. A good approximate expression of the R resistance matrix with the skin effect, is:

Rf() R

Where:

■

Ro is the DC resistance matrix.

■

Rs is the skin effect matrix.

+≅

f 1 j+()R

HSPICE® Signal Integrity User Guide 63 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Frequency-Dependent Matrices

The imaginary term depicts the correct frequency response at high frequency; however, it might cause significant errors for low-frequency applications. In the W Element, you can optionally exclude this imaginary term:

Wxxx i1 i2 ... iN iR o1 o2 ... oN oR N=val L=val INCLUDERSIMAG=NO

In contrast, the G (loss) conductance matrix is often approximated as:

Gf() G

-------------------------------- -

+≅

1 ffgd⁄()

Where:

■

Go models the shunt current due to free electrons in imperfect dielectrics.

■

Gd models the power loss due to the rotation of dipoles under the alternating field (C. A. Balanis, Advanced Engineering Electromagnetics, New York:

Wiley, 1989).

■

fgd is a cut-off frequency.

If you do not set fgd, or if you set fgd to 0, then G(f) keeps linear dependency on the frequency. In the W Element, the default fgd is zero (that is, G(f) does not use the fgd value).

You can specify an alternate value in the W Element statement:

Wxxx i1 i2 ... iN iR o1 o2 ... oN oR N=val L=val fgd=val

If you prefer to use the previous linear dependency, set fgd to 0.

Determining Matrix Properties

All matrices in Frequency-Dependent Matrices are symmetric.

■

The diagonal terms of L and C are positive, non-zero.

■

The diagonal terms of Ro, Rs, Go, and Gd are non-negative (can be zero).

■

Off-diagonal terms of the L, Ro impedance matrices are non-negative. Ro can have negative off-diagonal terms, but a warning appears. Negative

off-diagonal terms normally appear when you characterize Ro at a frequency higher than zero. Theoretically, R off-diagonal terms, because these might cause errors during analysis.

64 HSPICE® Signal Integrity User Guide

should not contain negative

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Wave Propagation

■

Off-diagonal terms of admittance matrices C, Go, and Gd are non-positive.

■

Off-diagonal terms of all matrices can be zero.

The elements of admittance matrices are related to the self/mutual admittances (such as those that the U Element generates):

∑

j 1=

self()mutual()⁄

Y–

mutual

In the preceding equations, Y stands for either C, Go, or Gd. A diagonal term of an admittance matrix is the sum of all self and mutual

admittance in this row . This term is larger (in absolute value) than the sum of all off-diagonal terms in its row or column. Admittance matrices are strictly diagonally dominant (except for a zero matrix).

You can obtain loop impedance matrix terms from the partial impedance matrix:

loop()

In the preceding equation, the o index denotes a reference node.

Wave Propagation

To illustrate the physical process of wave propagation and reflection in transmission lines, Figure 22 shows lines where the voltage step excites simple termination.

■

At the time t=t1, a voltage step from the e1 source, attenuated by the Z1 impedance, propagates along the transmission line.

■

At t=t2, the voltage wave arrives at the far end of the transmission line, is reflected, and propagates in the backward direction. The voltage at the load

end is the sum of the incident and reflected waves.

■

At t=t3, the reflected wave arrives back at the near end, is reflected again, and again propagates in the forward direction. The v oltage at the source end

is the sum of attenuated v oltage from the e1 source, the backward w ave, and the reflected forward w ave.

ij≠,=

partial()

Z–

partial()

Z–

partial()

HSPICE® Signal Integrity User Guide 65 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Wave Propagation

Figure 22 Propagation of a Voltage Step in a Transmission Line

t=t

x=0

x=l

0 2t 4t 6t 8t t

t1, t2, t

0 t 3t 5t 7t t

, t2, t

The surface plot in Figure 23 shows voltage at each point in the transmission line. The input incident propagates from the left (length = 0) to the right. You can observe both reflection at the end of the line (length = 1), and a reflected wave that goes backward to the near end.

66 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Wave Propagation

Figure 23 Surface Plot for the Transmission Line Shown in Figure 22

You can find more information about transmission lines in this resource: H.B. Bakoglu, Circuits, Interconnections and Packaging for VLSI. Reading, MA: Addison-Wesley, 1990.

Propagating a Voltage Step

This section is a summary of the process in Figure 22 to propagate a voltage step in a transmission line.

■

Signals from the excitation source spread-out in the termination networks, and propagate along the line.

■

As the forward wave reaches the far-end termination, it does the following:

•Reflects.

• Propagates backward.

• Reflects from the near-end termination.

• Propagates forward again.

• Continues in a loop.

■

The voltage at any point along the line , including the terminals, is a superposition of the forward and backward propagating waves.

HSPICE® Signal Integrity User Guide 67 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Wave Propagation

Figure 24 shows the system diagram for this process, where:

■

Wvr and Wvb are forward and backward matrix propagation functions for voltage waves.

■

T1, T2 stand for the near-end matrix transmission and reflection coefficients.

■

ΓΓ

(Gamma_1,Gamma_2) stand for the far-end matrix transmission

1, 2

and reflection coefficients.

Figure 24 System Model for Transmission Lines

N+1 conductor line R(f), L(f), G(f), C(f)

Signal Conductors

. . .

Reference conductor

0 lx

[v2] [v2]

[v2]

Termination

network2

. .

[e2]

. . .

[e2]

[e1]

1]1

[v1]

. . .

Termination

. .

[v1]

network1

This model reproduces the general relationship between the physical phenomena of wave propagation, transmission, reflection, and coupling in a distributed system. It can represent an arbitrarily-distributed system, such as:

■

Transmission line

■

Waveguide

■

Plane-wave propagation

68 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Wave Propagation

You can use this model for:

■

System analysis of distributed systems, or

■

Writing a macro solution for a distributed system without complicated mathematical derivations.

As shown in the figure, transmission lines and terminations form a feedback system. Because the feedback loop contains a delay, both the phase shift, and the sign of the feedback change periodically with the frequency. This causes oscillations in the frequency-domain response of the transmission lines, such as those shown in Example 30 on page 81.

Handling Line-to-Line Junctions

A special case occurs when the line terminates in another line. Figure 25 shows the system diagram for a line-to-line junction. You can use this diagram to:

■

Solve multi-layered plane-wave propagation problems.

■

Analyze common waveguide structures.

■

Derive generalized transmission and reflection coefficient formulas.

■

Derive scattering parameter formulas.

Figure 25 System Model for a Line-to-Line Junction

vr1

R1, L1, G1, C

. .

[v]

. .

[v]

+ +

vb1

HSPICE® Signal Integrity User Guide 69 X-2005.09

1 2

R2, L2, G2, C

. .

vr2

vb2

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

The Wvr and Wvb propagation functions describe how propagation (from one termination to another) affects a wave. These functions are equal for the

forward (Wvr) and backward (Wvb) directions. The off-diagonal terms of the propagation functions represent the coupling between conductors of a multi-

conductor line. As a wave propagates along the line, it experiences delay, attenuation, and

distortion (see Figure 26). Lines with frequency-dependent parameters (that is, all real lines) do not contain the frequency-independent attenuation component.

Figure 26 Propagation Function Transient Characteristics (unit-step

response)

Transient characteristic w

(t)

dependent

Attenuation

issues

LargerFrequency losses

Distortion

0Delay

Time, t

Using the W Element

The W Element is a multi-conductor lossy frequency-dependent transmission line. It provides advanced modeling capabilities for transmission lines. The W Element provides:

■

Ability to extract analytical solutions for AC and DC.

■

No limit on the number of coupled conductors.

■

No restriction on the structure of RLGC matrices; all matrices can be full.

■

No spurious ringing, such as the lumped model produces (see Figure 27 on

page 71).

■

Accurate modeling of frequency-dependent loss in the transient analysis.

70 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

■

Built-in 2D field solver, which you can use to specify a physical line shape.

Figure 27 Spurious Ringing in U Element

0.35

0.3

U element (300 segments)

W element

0.25

0.2

0.15

0.1

Transient Waveforms (V)

0.05 spurious ringing (U element)

-0.05 0 1020304050

Time (ns)

The W Element supports the following types of analysis:

■

Transient

■

RF analyses (HB, HPAC, HPACNOISE, PHASENOISE, LIN)

■

Parameter sweeps

■

Optimization

■

Monte-Carlo

Control Frequency Range of Interest for Greater Accuracy

This section describes the keywords you can use for achieving greater accuracy of the W Element by controlling the frequency of interest.

HSPICE® Signal Integrity User Guide 71 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

.OPTION RISETIME Setting

The W Element uses the .OPTION RISETIME parameter to estimate the frequency range of interest for the transient analysis of the W Element. Depending on the value of this parameter, analysis uses one of the following methods to determine the maximum frequency:

■

Positive value: The maximum frequency is the inv erse of the value that you specify.

■

No setting (recommended): Automatically determines the rise time from source statements. This method works for most cases. However, if the netlist contains the dependent source (which scales or shifts the frequency information), then you must explicitly set the rise time.

■

Zero: The internal W Element-bound algorithm computes the maximum frequency for each individual transmission line, and does not use the frequency information contained in source statements.

Note: If you specify DELAYOPT=3, then do not use the RISETIME option. When

DELAYOPT=3, the W Element automatically takes a broader frequency

range.

Use DELAYOPT Keyword for Higher Frequency Ranges

Long transmission lines fabricated in a high polymer insulator, such as PCB traces, show high losses in high frequencies due to dielectric loss. In such cases, the propagation delay of the system becomes a non-constant function of frequency. To take this phenomenon accurately, beginning with the 2003.09 release of HSPICE, a novel pre-process function was introduced for constructing W Element transient (recursive convolution) model with a higher level of accuracy. To activate this new function, you can add the DELAYOPT keyword to the W Element instance line. You can use DELAYOPT=0|1|2 to deactivate, activate, and automatic determination, respectively. The default value is 0 (deactivate). If this function is deactivated, the W Element behaves identical to the previous ve rsions.

Beginning with the 2004.03 release, DELAYOPT=3 was introduced, which achieves a higher level of accuracy up to a tens of GHz operation and involves harmonics up to THz order. With this option, line length limits are remov ed, which frees the simulation from segmenting, and allows independence in the behavior of the risetime option setting. A setting of DELAYOPT=3 automatically detects whether or not frequency-dependent phenomena need to be recorded, which makes it identical to the DELAYOPT=0 option if it produces a high enough accuracy.

72 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

Note: The DELAYOPT=3 option activates additional evaluation functions in

transient analysis, which might take longer CPU time.

Use DCACC Keyword for Lower Frequency Ranges

Beginning with the 2005.03 release, The W Element takes an additional step in making a time domain model check the accuracy of low frequency and DC coverage. And it automatically adds a few rational function terms if necessary. This process may cause slight additional computational cost and slight difference in element behavior in DC offset than in previous versions. Should you choose to use this conventional behavior, set DCACC=0 in the W Element instance or model line to deactivate this process.

W Element Time-Step Control in Time Domain

This section describes using static and dynamic time-step controls in the time domain.

Using Static Time-Step Control

The W Element provides accurate results with just one or two time steps per excitation transient (0.1 ns in Figure 27 on page 71). Like the T Element, the W Element supports the TLINLIMIT option. The TLINLIMIT=0 default setting enables special breakpoint building, which limits the maximum time step b y the smallest transmission line delay in the circuit. This improves transient accuracy for short lines, but reduces efficiency. Setting TLINLIMIT=1 disables this special breakpoint building.

Longer transmission lines might experience prolonged time intervals when nothing happens at the terminals, while the wave propagates along the line. If you increase the time step, the accuracy of the simulation decreases when the wave reaches the terminal. To prevent this for longer lines excited with short pulses, set .OPTION DELMAX to limit the time step to between 0.5 and 1 of the excitation transient.

Using Dynamic Time-Step Control

Static time step control achieves certain accuracy by setting static breakpoints . The TLINLIMIT=0 option limits the maximum time step by the minimum transmission line delay, which results in poor performance for the cases with ultra-short delay transmission lines. In this case, too many redundant time

HSPICE® Signal Integrity User Guide 73 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

points are calculated, especially when the transmission line terminal signals do not vary rapidly. The same problem exists with the DELMAX option where time steps are ev enly set in spite of terminal signal variation. This is inefficient.

In the 2004.09 release, the WACC option was added to solve this problem by providing dynamic step control of W Element transient analysis. Setting WACC to a positive value removes the static breakpoints and the necessary time points are set dynamically according to the variations in terminal currents and voltages.

The WACC option has the following syntax:

.OPTION WACC=value

Where WACC is a non-negative real value. It can be set between 0.0 and 10.0. When WACC is positive, the new method is activated. The default value is 0.0.

Larger values result in higher performance with lower accuracy, while smaller values result in lower performance with better accuracy. Use WACC=1.0 for normal simulation and WACC=0.1 for an accurate simulation. When WACC=0.0, the conventional step control method is used.

The WACC option has a higher priority than the TLINLIMIT option. It is only when WACC=0.0 can the TLINLIMIT option limit the maximum time step by the minimum transmission line delay. The DELMAX option has a higher priority than the WACC option. You can further limit the time step by setting the DELMAX option in addition to the WACC option.

74 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

Input Syntax for the W Element

Syntax:

Wxxx i1 i2 ... iN iR o1 o2 ... oN oR N=val L=val + <RLGCMODEL=name or RLGCFILE=name or UMODEL=name + FSMODEL=name or TABLEMODEL=name or SMODEL=name> + [ INCLUDERSIMAG=YES|NO FGD=val ] [ DELAYOPT=0|1|2 ] + <NODEMAP=XiYj...> <NOISE=[1|0]> <DTEMP=val>

Parameter Description

N Number of signal conductors (excluding the reference

conductor).

i1...iN Node names for the near-end signal-conductor terminal

(Figure 28 on page 77).

iR Node name for the near-end reference-conductor terminal. o1... oN Node names for the far-end signal-conductor terminal

(Figure 28 on page 77). oR Node name for the far-end reference-conductor terminal. L Length of the transmission line. RLGCMODEL Name of the RLGC model. RLGCFILE Name of the external file with RLGC parameters. (See Input

Model 1: W Element, RLGC Model on page 78.)

UMODEL Name of the U model. (See Input Model 2: U Element, RLGC

Model on page 84.)

FSMODEL Name of the field solver model. TABLEMODEL Name of the frequency-dependent tabular model. SMODEL Name of the S mo del. (See Input Model 5: S Model on page 92.) INCLUDERSIMAG Imaginary term of the skin effect to be considered. The default

value is YES. (See Frequency-Dependent Matrices on

page 63.)

HSPICE® Signal Integrity User Guide 75 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

Parameter Description

FGD Specifies the cut-off frequency of dielectric loss. (See Handling

the Dielectric-loss Matrix on page 85.)

DELAYOPT Deactivates (0), activates (1) or determines automatically(2).

The default is 0. NODEMAP String that assigns each index of the S parameter matrix to one

of the W Element terminals. This string must be an arra y 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 indica te f ar end (output side) terminal of the W element.

The default v alue is NODEMAP = I1I2I3...InO1O2O3...On.

NOISE Activates thermal noise.

•

1: element generates thermal noise

•

0 (default): element is considered noiseless

DTEMP Temperature difference between the element and the circuit,

expressed in °C. The default is 0.0. Element temperature is calculated as:

T = Element temperature (°K)

= 273.15 (°K) + circuit temperature (°C)

+ DTEMP (°C)

Where circuit temperature is specified using either the statement, or by sweeping the global TEMP variab le in

.TEMP

.DC,

.AC, or .TRAN statements.

When a circuit temperature is set by 25 °C unless you use default to 27 °C.

.TEMP statement or TEMP variable is not used, the

.OPTION TNOM, which defaults to

.OPTION SPICE, which raises the

76 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

The W Element supports four different formats to specify the transmission line properties:

■

Model 1: RLGC-Model specification

• Internally specified in a .MODEL statement.

• Externally specified in a different file.

■

Model 2: U-Model specification

• RLGC input for up to five coupled conductors

• Geometric input (planer, coax, twin-lead)

• Measured-parameter input

• Skin effect

■

Model 3: Built-in field solver model

■

Model 4: Frequency-dependent tabular model.

■

Model 5: S model specification

• S parameters specified by an S model

• Valid only for transmission line-based S parameters.

Figure 28 Terminal Node Numbering

N+1 conductor line

[i2]

2.1

[i2]

2.2

. . .

[i2]

2.N 2’

1.1

1.2

1.N

[i1]

1]1

[i1]

[v1]

. . .

[i1]

[v1]

1’

R(f), L(f), G(f), C(f)

Signal Conductors

[v2] [v2]

. . .

[v2]

Reference conductor

0 lx

Normally, you can specify parameters in the W Element card in any order. Specify the number of signal conductors, N, after the list of nodes. You can intermix the nodes and parameters in the W Element card.

HSPICE® Signal Integrity User Guide 77 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

You can specify only one RLGCMODEL, FSMODEL, UMODEL, or RLGCFILE in a single W Element card.

Input Model 1: W Element, RLGC Model

Equations and Parameters on page 62 describes the inputs of the W Element

per unit length matrices:

■

Rs (skin effect)

■

Gd (dielectric loss)

The W Element does not limit any of the following parameters:

■

Number of coupled conductors.

■

Shape of the matrices.

■

Line loss.

■

Length or amount of frequency dependence.

The RLGC text file contains frequency-dependent RLGC matrices per unit length.

The W Element also handles frequency-independent RLGC, and lossless (LC) lines. It does not support RC lines.

Because RLGC matrices are symmetrical, the RLGC model specifies only the lower triangular parts of the matrices. The syntax of the RLGC model for the W Element is:

.MODEL name W MODELTYPE=RLGC N=val Lo=matrix_entries + Co=matrix_entries [ Ro=matrix_entries Go=matrix_entries + Rs=matrix_entries Gd=matrix_entries Rognd=val + Rsgnd=val Lgnd=val ]

78 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

Parameter Description

N Number of conductors (same as in the element card). L

gnd

Ω

---- m

Ω

---------------- -

DC inductance matrix, per unit length .

DC capacitance matrix, per unit length .

DC resistance matrix, per unit length .

DC shunt conductance matrix, per unit length .

Skin effect resistance matrix, per unit length .

mHz

Dielectric loss conductance matrix, per unit length .

DC inductance value, per unit length for grounds (reference

---------------- mHz⋅

---- m

line).

ognd

sgnd

DC resistance value, per unit length for ground .

Skin effect resistance value, per unit length for ground .

Ω

---- m

Ω

---------------- mHz

HSPICE® Signal Integrity User Guide 79 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

The following input netlist file shows RLGC input for the W Element:

* W-Element example, four-conductor line W1 N=3 1 3 5 0 2 4 6 0 RLGCMODEL=example_rlc l=0.97 V1 1 0 AC=1v DC=0v pulse(4.82v 0v 5ns 0.1ns 0.1ns 25ns) .AC lin 1000 0Hz 1GHz .DC v1 0v 5v 0.1v .tran 0.1ns 200ns

* RLGC matrices for a four-conductor lossy .MODEL example_rlc W MODELTYPE=RLGC N=3 + Lo= + 2.311e-6 + 4.14e-7 2.988e-6 + 8.42e-8 5.27e-7 2.813e-6 + Co= + 2.392e-11 + -5.41e-12 2.123e-11 + -1.08e-12 -5.72e-12 2.447e-11 + Ro= + 42.5 + 0 41.0 + 0 0 33.5 + Go= + 0.000609 + -0.0001419 0.000599 + -0.00002323 -0.00009 0.000502 + Rs= + 0.00135 + 0 0.001303 + 0 0 0.001064 + Gd= + 5.242e-13 + -1.221e-13 5.164e-13 + -1.999e-14 -7.747e-14 4.321e-13 .end

The following three figures show plots of the simulation results:

■

Figure 29 shows DC sweep

■

Figure 30 shows AC response

■

Figure 31 shows transient waveforms.

These figures also demonstrate that the transmission line behavior of interconnects has a significant and complicated effect on the integrity of a signal. This is why it is v e ry important to accurately model transmission lines when you verify high-speed designs.

80 HSPICE® Signal Integrity User Guide

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Figure 29 Simulation Results: DC Sweep

1.4

1.2

Using the W Element

0.8

0.6

0.4

dc Transfer Curves (V)

0.2

-0.2 012345

V1 (V)

Figure 30 Simulation Results: AC Response

Frequency Responses (V)

0 200 400 600 800 1000

Frequency (MHz)

HSPICE® Signal Integrity User Guide 81 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

Figure 31 Simulation Results: Transient Waveforms

Transient Waveforms (V)

-2

-4 0 50 100 150 200

Time (ns)

Specifying the RLGC Model in an External File

You can also specify RLGC matrices in a RLGC file. Its file format is more restricted than the RLGC model; for example:

■

You cannot include any parameters.

■

The file does not support ground inductance and resistance.

Note: This format does not provide any adv antage ov er the RLGC model so do

not use it unless you already have an RLGC file. It is supported for backward-compatibility.

The RLGC file only specifies the lower-triangular parts of the matrices and is order-dependent. Its parameters are in the following order:

Table 5 Parameters in RLGC File for W Element

Parameter Description

N Number of conductors (same as in the element card). L

DC inductance matrix, per unit length .

DC capacitance matrix, per unit length .

82 HSPICE® Signal Integrity User Guide

---- m

X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Table 5 Parameters in RLGC File for W Element

Using the W Element

Ro (Optional)

DC resistance matrix, per unit length .

Go (Optional)

DC shunt conductance matrix, per unit length .

Rs (Optional)

Skin effect resistance matrix, per unit length .

Gd (Optional)

Dielectric loss conductance matrix, per unit length .

---- m

Ω

---- m

Ω

---------------- mHz

---------------- mHz⋅

Note: You can skip the optional parameters, because they default to zero. But

if you specify an optional parameter, then you must specify all preceding parameters, even if they are zero.

An asterisk (*) in an RLGC file comments out everything until the end of that line. You can use any of the following characters to separate numbers:

space tab newline , ; ( ) [ ] { }

This RLGC file is for the same netlist example used for the RLGC model in the previous section:

* W- Element example, four-conductor line

W1 N=3 1 3 5 0 2 4 6 0 RLGCfile=example.rlc l=0.97 V1 1 0 AC=1v DC=0v pulse(4.82v 0v 5ns 0.1ns 0.1ns 25ns)

.AC lin 1000 0Hz 1GHz .DC v1 0v 5v 0.1v .tran 0.1ns 200ns

.end

Calls this example.rlc file:

* RLGC parameters for a four-conductor lossy * frequency-dependent line * N (number of signal conductors)

HSPICE® Signal Integrity User Guide 83 X-2005.09

3: Modeling Coupled Transmission Lines Using the W Element

Using the W Element

* Lo

2.311e-6

4.14e-7 2.988e-6

8.42e-8 5.27e-7 2.813e-6

* Co

2.392e-11

-5.41e-12 2.123e-11

-1.08e-12 -5.72e-12 2.447e-11

* Ro

42.5 0 41.0 0 0 33.5

* Go

0.000609

-0.0001419 0.000599

-0.00002323 -0.00009 0.000502

* Rs

0.00135 0 0.001303 0 0 0.001064

* Gd

5.242e-13

-1.221e-13 5.164e-13

-1.999e-14 -7.747e-14 4.321e-13

The RLGC file format does not support scale suffixes, such as:

n (10^-9) or p (10^-12)

Input Model 2: U Element, RLGC Model

The W Element accepts the U model as an input to provide backward compatibility with the U Element. It also uses the geometric and measuredparameter interfaces of the U model.

To use the W Element with the U model on the W Element card, specify:

Umodel=U-model_name

84 HSPICE® Signal Integrity User Guide

X-2005.09

Synopsys HSPICE USER MANUAL

Specifications and Main Features

Frequently Asked Questions

User Manual

Contents

Inside This Manual

The HSPICE Documentation Set

Searching Across the HSPICE Documentation Set

Other Related Publications

Conventions

Customer Support

Preparing for Simulation

1Introduction

Signal Integrity Problems

Analog Side of Digital Logic

Optimizing TDR Packaging

Using TDR in Simulation

TDR Optimization Procedure

Simulating Circuits with Signetics Drivers

Simulating Circuits with Xilinx FPGAs

Syntax for IOB (xil_iob) and IOB4 (xil_iob4)

Ground-Bounce Simulation

Coupled Line Noise

S Parameter Model

2S Parameter Modeling Using the S Element

Using the Scattering Parameter Element

S Element Syntax

S Model Syntax

S Element Data File Model Examples

S Element Noise Model

Two-Port Noise Parameter Support in Touchstone Files

Input Interface

Output Interface

Notifications and Limitations

Multiport Noise Model for Passive Systems

Input Interface

Output Interface

Notifications and Limitations

Mixed-Mode S Parameters

Relating Voltage and Current Waves to Nodal Waves

Characterizing Differential Data Transfer Systems

Deriving a Simpler Set of Voltage and Current Pairs

Using the Mixed-Mode S Parameters (S Element)

Small-Signal Parameter Data-Table Model

Mixed-Mode S Parameter Netlist Examples

SP Model Syntax

Equations and Parameters

Frequency-Dependent Matrices

Determining Matrix Properties

Wave Propagation

Propagating a Voltage Step

Handling Line-to-Line Junctions

Using the W Element

Control Frequency Range of Interest for Greater Accuracy

.OPTION RISETIME Setting

Use DELAYOPT Keyword for Higher Frequency Ranges

Use DCACC Keyword for Lower Frequency Ranges

W Element Time-Step Control in Time Domain

Using Static Time-Step Control

Using Dynamic Time-Step Control

Input Syntax for the W Element

Input Model 1: W Element, RLGC Model

Specifying the RLGC Model in an External File

Input Model 2: U Element, RLGC Model