Appendix. RF Transient Simulator. Page 1

Save this PDF as:

Size: px
Start display at page:

Transcription

1 Appendix RF Transient Simulator Page 1

2 RF Transient/Convolution Simulation This simulator can be used to solve problems associated with circuit simulation, when the signal and waveforms involved are modulated with complex signals. Such signals represent the primary types of signals found in modern RF communication systems. The most traditional simulation solutions are based on SPICE or SPICE-like time domain algorithms. The Transient and convolution simulators are SPICE-like in their operation. They solve a set of integro-differential equations that express the time dependence of the currents and voltages of the circuit under analysis. The result is a nonlinear analysis with respect to time and, possibly, a swept variable. These simulation techniques assume that the input stimulus can be an arbitrary baseband signal so the solution v(t) must also be assumed to be a baseband signal. This means that any high frequency carrier must be represented as baseband signals and must therefore be sampled at rates significantly higher than the most significant harmonic frequency. For example, assume a 5GHz signal with significant 3 rd harmonic. To satisfy the basic Nyquist criteria, the sampling frequency must be greater than 30GHz. To obtain reasonable accuracy from the integration algorithm, a sampling frequency of 100GHz is a more realistic value. Now assume that the carrier is modulated with a symbol rate of 100 khz, and that we want to simulate the circuit for 500 symbols. This means that we desire a total simulation time of 5 ms. However, the high carrier frequency dictates the step size that must be at least 10 ps or smaller. This means then that the circuit simulator must solve the circuit equations and outputs solutions at over 500 million time points. Features of Transient Analysis Analyze low and high frequencies, linear and non-linear large circuits in the time domain Verify transient behavior like start-up time in oscillators, step-function responses in filters, pulsed RF network responses, high speed digital and switching circuits and more. Improved convergence for large and highly non-linear circuits. Time-to-frequency domain transformation allows RF designers to view the output results (such as IP3) in the frequency domain. The main difference between the transient and convolution option lies in how each analysis characterizes the distributed and frequency-dependent elements of a circuit. Page 2

3 High-Frequency Spice Analysis A High-Frequency-Spice-Analysis is performed entirely in the time-domain, and so is unable to account for the frequency-dependent behavior of distributed elements such as microstrip elements, S-parameter elements, and so on. Therefore in a transient analysis, such elements must be represented by simplified, frequency-independent models such as lumped equivalents, transmission lines with constant loss and no dispersion, short circuits, open circuits, and the like. These assumptions and simplifications are usually very reasonable at low frequencies. Features of High-Frequency SPICE Directly uses high-frequency time-models for microstrip lines, bends, gaps, etc. Used to analyze the steady state response of mixes, oscillators, amplifiers and so on. Frequency-dependent elements are modeled with approximations that neglect some of the frequency-dependent effects, such as dispersion and high frequency loss, resulting in faster simulations this is accurate enough for electrically small components (ICs). Convolution Analysis A convolution analysis, on the other hand, represents all the distributed elements in the frequency domain and hence accounts for their frequency dependent behavior. The characterization of many distributed elements is best accomplished in the frequency domain, because the exact time-domain equivalents for these elements cannot always be obtained. Convolution converts the frequency-domain information from all the distributed elements to the time-domain, effectively resulting in the impulse response of those elements. The timedomain-input signals at the element s terminals are convolved with the impulse-response of the element to yield the output signals. Elements that have exact lumped equivalent models including nonlinear elements are characterized entirely in the time domain without using the impulse responses. Features of Convolution Simulation For more accurate analysis of the discontinuities and for more accurate frequency-domain models with dispersion effects and high frequency loss. Convolution simulator results in accurate high frequency results at the expense of longer simulation times. Handles circuits that contain distributed elements and S-Parameter data used for components. It can accurately analyze circuit startup and transient conditions at low- and high frequencies, where the effects of dispersion and discontinuities are significant (for electrically big components on PCB-boards). Extension of High-Frequency-SPICE. Basic time step and convergence algorithms and non-linear models are the same; only modeling of Frequency-dependent linear devices is enhanced. Page 3

4 High-Frequency Spice versus Convolution Always check the settings for convolution. To use only High-Frequency Spice, you must turn off (Advanced button) the Use approximate models setting in the transient controller. Almost every component in ADS has a non-convolution representation for High- Frequency Spice use. The primary exceptions are S-parameter based elements where the user either enters the S-parameter directly or reads them from a file. During High- Frequency Spice simulation, those components are simulated using just their DC response. For this reason, all S-parameter based elements should have their DC response correctly defined. In general, convolution simulation results in more accuracy at the expense of longer simulation time, depending upon how detailed the impulse response may be. Convolution is only performed on linear and time invariant elements. You don t use nor need convolution on bias-dependent transistors and other non-linear elements. Convolution is a modeling issue. The real issue regarding simulation time is the ratio of convolution elements to non-linear elements. If non-linear devices greatly outnumber the convolution elements, then you ll never notice the time needed for convolution. How the High-Frequency-Spice and Convolution Simulator Operate 1. The user specifies a time-sweep range, Tolerances and iteration limits: 2. A DC analysis is performed to determine the system solution at time zero. 3. Inside the simulator, a breakpoint table is constructed to deal with frequency-domaindevices and data. Independent source waveforms frequently have sharp transitions that may not normally coincide with the time step calculated by the program. Such is the case with the piecewise linear sources. The breakpoint table contains a sorted list of all the transition points of the independent sources. During the simulation, whenever the next time point is sufficiently close to one of the breakpoints, the time step is adjusted to land exactly at the breakpoint. This prevents unnecessary time-step reductions in the vicinity of the transitions. Page 4

5 4. An internal control variable updates the current time and the value of the independent sources are calculated at that time. 5. An attempt is made to solve the system of equations through numerical integration and a finite number of Newton-Raphson iterations. If the number of iterations exceeds Max iterations per time point, then the time step is reduced by a factor of Integration coefficient mu divided by 8. If the new time step is acceptable, the analysis is repeated from step 4. If the Integration coefficient mu =0, backward-euler numerical integration is used. Otherwise, trapezoidal integration is used. 6. Following convergence, the local truncation error is calculated. The default trapezoidal integration method is used to estimate the error, unless Gear s method is selected. 7. The time step interval is calculated. By default, the time step is computed for transient analysis by means of the truncation error estimate method. 8. The error tolerance is compared with the value in the Local truncation over-est factor. If the error is within acceptable limits, the results are stored and analysis continues at the next time point. Otherwise, the analysis is repeated at a smaller time step. 9. Steps 3 through 9 are repeated until the user-specified time-sweep range has been analyzed. Integration Method Like SPICE, this simulator uses the trapezoidal integration method as the default method for calculating derivatives at each time step t in the simulation. For most circuits, this method will succeed. Trapezoidal integrates between time points by assuming line segments connect them. The local truncation error is then related to the difference between the areas determined by the present and previous time point.. For those few that do not, the simulator also supports Gear s backward difference method. v In this equation, the index k is called the order of the integration. Page 5

6 Gear s integrates by assuming that the time points are connected by a polynomial curve. The order of the polynomial is controlled by the Max Gear order parameter. Lower-order polynomials tend to create greater truncation error, while higher-order polynomials can become unstable. For most circuits, Gear s method is no more accurate then the trapezoidal integration technique. However, if a circuit analysis fails to converge, Gear s method may succeed where trapezoidal integration fails. If Max Gear order is set to a number between 2 and 6, the simulator will use Gear s method along with an adaptive step size algorithm that picks the largest possible step size at each point in the simulation. For each time step, the order of Gear s method will be chosen (up to the value of Max Gear order) to maintain accuracy with the largest possible time step. This potentially speeds up simulations with no loss in accuracy. Memory Requirements and Simulation Time With large circuit transient simulation, memory requirement grows linearly with the number of transistors in the circuit. ADS use roughly one megabyte per 100 transistors. Simulation time grows superlinearly with the number of transistors; N. Time of simulation grows N 1.2. Therefore, if you double the transistors in a circuit, it will take 2.3 times the original simulation time. Example: If we have 1000 nodes in a circuit, the full matrix size would be 1000 * 1000 = 1,000,000 entries. But this full matrix is presupposed on the fact, that every node is connected to every other node. In any practical electrical circuit, any given node is normally connected to just a handful of other nodes; there is no connection to all of the other nodes. Sparse matrix techniques allow taking advantage of this fact and we only have to keep track of those nodes that are actually connected to other nodes. This allows us to effectively store a matrix with 1000 nodes using only 10,000 entries (1% of the full size). This makes the simulator s use of memory much more efficient. The N 1.2 factor is due to the way the sparse matrix techniques work in solving for the solution. Parasitic extraction of interconnects resistance and capacitance from an IC layout of a typical large circuit with N non-linear devices will have 5-10times N passive components. Therefore a rule of thumb is that extraction from the layout generates about 10 passives (RC) per transistor. This is after model reduction of the passives. Without model reduction, an extraction yields 1000 passives (RC) per transistor. Model reduction deduces this by 100 times. When combining digital and analog circuits on one chip, parasitic and substrate coupling becomes an issue. In this case we are talking about millions of transistors on one chip. Any Spice-type time domain simulator runs out of steam past transistor point. If we model the substrate coupling, every transistor will have about 10 passive parasitic. Therefore it is still a major and unresolved problem, on how to simulate and verify the whole chip using SPICE tool. Page 6

7 Convolution Tab Settings Recent improvements to the ADS Transient simulator have greatly improved the results of Convolutions anaysis. For that reason, some previous settings are now obsolete and it is recommended that the tolerance settings be left in Auto mode. Here are the impulse response truncation factors for the three settings: Relax: ImpRelTrunc = 1e-2 ImpAbsTrunc = 1e-5 Auto: ImpRelTrunc = 1e-4 ImpAbsTrunc = 1e-7 Strict: ImpRelTrunc = 1e-6 ImpAbsTrunc = 1e-8 Enforcing passivity - This can be turned on for linear frequency domain components which are simulated using discrete mode convolution. Similarly, if EnforcePassivity=yes in a SnP component, passivity will be enforced in that particular device. The EnforcePassivity setting of SnP component overwrites the ImpEnforcePassivity setting of the transient controller in an individual device. NOTE designs from a previous release uses PWL Continuous mode, ADS 2008 automatically sets the parameter to Discrete mode. Approximate models this selection uses models that, although somewhat less accurate, can provide faster simulations. These approximations neglect effects such as frequency-dependent loss and dispersion, but include the basic delay and impedance. These models are the default, if no convolution license is available. Save impulse spectrum - saves the impulse response, its FFT, and the original spectrum to a dataset when discrete mode convolution is used in transient analysis. NOTE on Noncausal Frequency Responses: In ADS 2008, the simulator produces warnings when non-causality is detected and it also attempts to eliminate the problem. In general, the supports user-defined models that can have any impedance, including nonphysical or noncausal components for which there is no correct answer. If a component has a constant reactance that does not vary with frequency (or has a nonzero reactance at DC), then the component is mathematically nonphysical. In these cases, the simulator may produce an answer that may not be physically realistic. To eliminate this problem, change the component's definition. Refer to the documentation (manuals) for more details Transient analysis and settings. Page 7

8 Using measured and simulated S-Parameter Data The ability to handle convolution-based devices allows the user of measured or simulated S- parameter data to describe a wide variety of devices and circuits. A dataset or file containing the S-parameter values can be used to integrate the frequency response into a time-domain simulation. This adds a tremendous amount of flexibility to the number and types of devices and circuits that can be used in a simulation. When S-Parameter data is used, it is important that the frequency response be adequately sampled over the entire bandwidth to ensure negligible interpolation errors when the impulse response is calculated. The Max Frequency parameter should never be set to a value that is greater then the maximum S-parameter data frequency. Doing so will lead to erroneous results as the available data would have to be extrapolated. S-parameter data must also extend all the way down to DC. Page 8

Appendix. Harmonic Balance Simulator. Page 1

Appendix Harmonic Balance Simulator Page 1 Harmonic Balance for Large Signal AC and S-parameter Simulation Harmonic Balance is a frequency domain analysis technique for simulating distortion in nonlinear

Fundamentals of RF Design RF Back to Basics 2015

Fundamentals of RF Design 2015 Updated January 1, 2015 Keysight EEsof EDA Objectives Review Simulation Types Understand fundamentals on S-Parameter Simulation Additional Linear and Non-Linear Simulators

Advanced Design System - Fundamentals. Mao Wenjie

Advanced Design System - Fundamentals Mao Wenjie wjmao@263.net Main Topics in This Class Topic 1: ADS and Circuit Simulation Introduction Topic 2: DC and AC Simulations Topic 3: S-parameter Simulation

Analysis and Design of Autonomous Microwave Circuits

Analysis and Design of Autonomous Microwave Circuits ALMUDENA SUAREZ IEEE PRESS WILEY A JOHN WILEY & SONS, INC., PUBLICATION Contents Preface xiii 1 Oscillator Dynamics 1 1.1 Introduction 1 1.2 Operational

Evaluation of Package Properties for RF BJTs

Application Note Evaluation of Package Properties for RF BJTs Overview EDA simulation software streamlines the development of digital and analog circuits from definition of concept and estimation of required

Window Functions And Time-Domain Plotting In HFSS And SIwave

Window Functions And Time-Domain Plotting In HFSS And SIwave Greg Pitner Introduction HFSS and SIwave allow for time-domain plotting of S-parameters. Often, this feature is used to calculate a step response

LIMITATIONS IN MAKING AUDIO BANDWIDTH MEASUREMENTS IN THE PRESENCE OF SIGNIFICANT OUT-OF-BAND NOISE

LIMITATIONS IN MAKING AUDIO BANDWIDTH MEASUREMENTS IN THE PRESENCE OF SIGNIFICANT OUT-OF-BAND NOISE Bruce E. Hofer AUDIO PRECISION, INC. August 2005 Introduction There once was a time (before the 1980s)

915 MHz Power Amplifier. EE172 Final Project. Michael Bella

915 MHz Power Amplifier EE17 Final Project Michael Bella Spring 011 Introduction: Radio Frequency Power amplifiers are used in a wide range of applications, and are an integral part of many daily tasks.

2. There are many circuit simulators available today, here are just few of them. They have different flavors (mostly SPICE-based), platforms,

1. 2. There are many circuit simulators available today, here are just few of them. They have different flavors (mostly SPICE-based), platforms, complexity, performance, capabilities, and of course price.

April 26, 2018 Wendem Beyene UIUC ECE 546 Statistical Link Modeling Review of Basic Techniques What is a High-Speed Link? 1011...001 TX Channel RX 1011...001 Clock Clock Three basic building blocks: Transmitter,

An Oscillator Puzzle, An Experiment in Community Authoring

The Designer s Guide Community downloaded from An Oscillator Puzzle, An Experiment in Community Authoring Ken Kundert Designer s Guide Consulting, Inc. Version 2, 1 July 2004 Certain oscillators have been

Validation & Analysis of Complex Serial Bus Link Models

Validation & Analysis of Complex Serial Bus Link Models Version 1.0 John Pickerd, Tektronix, Inc John.J.Pickerd@Tek.com 503-627-5122 Kan Tan, Tektronix, Inc Kan.Tan@Tektronix.com 503-627-2049 Abstract

Department of Electronic Engineering NED University of Engineering & Technology. LABORATORY WORKBOOK For the Course SIGNALS & SYSTEMS (TC-202)

Department of Electronic Engineering NED University of Engineering & Technology LABORATORY WORKBOOK For the Course SIGNALS & SYSTEMS (TC-202) Instructor Name: Student Name: Roll Number: Semester: Batch:

Simulation of Radio Frequency Integrated Circuits

Simulation o Radio Frequency Integrated Circuits Based on: Computer-Aided Circuit Analysis Tools or RFIC Simulation: Algorithms, Features, and Limitations, IEEE Trans. CAS-II, April 2000. Outline Introduction

2005 Modelithics Inc.

Precision Measurements and Models You Trust Modelithics, Inc. Solutions for RF Board and Module Designers Introduction Modelithics delivers products and services to serve one goal accelerating RF/microwave

An Initial Case Study for BIRD95: Enhancing IBIS for SSO Power Integrity Simulation

An Initial Case Study for BIRD95: Enhancing IBIS for SSO Power Integrity Simulation Also presented at the January 31, 2005 IBIS Summit SIGRITY, INC. Sam Chitwood Raymond Y. Chen Jiayuan Fang March 2005

Efficiently simulating a direct-conversion I-Q modulator

Efficiently simulating a direct-conversion I-Q modulator Andy Howard Applications Engineer Agilent Eesof EDA Overview An I-Q or vector modulator is a commonly used integrated circuit in communication systems.

Ansys Designer RF Training Lecture 3: Nexxim Circuit Analysis for RF

Ansys Designer RF Solutions for RF/Microwave Component and System Design 7. 0 Release Ansys Designer RF Training Lecture 3: Nexxim Circuit Analysis for RF Designer Overview Ansoft Designer Advanced Design

A Simplified Extension of X-parameters to Describe Memory Effects for Wideband Modulated Signals

A Simplified Extension of X-parameters to Describe Memory Effects for Wideband Modulated Signals Jan Verspecht*, Jason Horn** and David E. Root** * Jan Verspecht b.v.b.a., Opwijk, Vlaams-Brabant, B-745,

THE SPICE BOOK. Andrei Vladimirescu. John Wiley & Sons, Inc. New York Chichester Brisbane Toronto Singapore

THE SPICE BOOK Andrei Vladimirescu John Wiley & Sons, Inc. New York Chichester Brisbane Toronto Singapore CONTENTS Introduction SPICE THE THIRD DECADE 1 1.1 THE EARLY DAYS OF SPICE 1 1.2 SPICE IN THE 1970s

2.1 BASIC CONCEPTS Basic Operations on Signals Time Shifting. Figure 2.2 Time shifting of a signal. Time Reversal.

1 2.1 BASIC CONCEPTS 2.1.1 Basic Operations on Signals Time Shifting. Figure 2.2 Time shifting of a signal. Time Reversal. 2 Time Scaling. Figure 2.4 Time scaling of a signal. 2.1.2 Classification of Signals

EE228 Applications of Course Concepts. DePiero

EE228 Applications of Course Concepts DePiero Purpose Describe applications of concepts in EE228. Applications may help students recall and synthesize concepts. Also discuss: Some advanced concepts Highlight

Filtering in the spatial domain (Spatial Filtering)

Filtering in the spatial domain (Spatial Filtering) refers to image operators that change the gray value at any pixel (x,y) depending on the pixel values in a square neighborhood centered at (x,y) using

Introduction. In the frequency domain, complex signals are separated into their frequency components, and the level at each frequency is displayed

SPECTRUM ANALYZER Introduction A spectrum analyzer measures the amplitude of an input signal versus frequency within the full frequency range of the instrument The spectrum analyzer is to the frequency

AC Analyses. Chapter Introduction

Chapter 3 AC Analyses 3.1 Introduction The AC analyses are a family of frequency-domain analyses that include AC analysis, transfer function (XF) analysis, scattering parameter (SP, TDR) analyses, and

Introduction to RF Simulation and Its Applications

Introduction to RF Simulation and Its Applications by Kenneth S. Kundert Presenter - Saurabh Jain What will he talk about? Challenges for RF design and simulations RF circuit characteristics Basic RF building

ME scope Application Note 01 The FFT, Leakage, and Windowing

INTRODUCTION ME scope Application Note 01 The FFT, Leakage, and Windowing NOTE: The steps in this Application Note can be duplicated using any Package that includes the VES-3600 Advanced Signal Processing

EECS 216 Winter 2008 Lab 2: FM Detector Part I: Intro & Pre-lab Assignment

EECS 216 Winter 2008 Lab 2: Part I: Intro & Pre-lab Assignment c Kim Winick 2008 1 Introduction In the first few weeks of EECS 216, you learned how to determine the response of an LTI system by convolving

Gain Compression Simulation

Gain Compression Simulation August 2005 Notice The information contained in this document is subject to change without notice. Agilent Technologies makes no warranty of any kind with regard to this material,

(i) Understanding the basic concepts of signal modeling, correlation, maximum likelihood estimation, least squares and iterative numerical methods

Tools and Applications Chapter Intended Learning Outcomes: (i) Understanding the basic concepts of signal modeling, correlation, maximum likelihood estimation, least squares and iterative numerical methods

Substrate Coupling in RF Analog/Mixed Signal IC Design: A Review

Substrate Coupling in RF Analog/Mixed Signal IC Design: A Review Ashish C Vora, Graduate Student, Rochester Institute of Technology, Rochester, NY, USA. Abstract : Digital switching noise coupled into

How to Utilize a Windowing Technique for Accurate DFT

How to Utilize a Windowing Technique for Accurate DFT Product Version IC 6.1.5 and MMSIM 12.1 December 6, 2013 By Michael Womac Copyright Statement 2013 Cadence Design Systems, Inc. All rights reserved

EET 223 RF COMMUNICATIONS LABORATORY EXPERIMENTS

EET 223 RF COMMUNICATIONS LABORATORY EXPERIMENTS Experimental Goals A good technician needs to make accurate measurements, keep good records and know the proper usage and limitations of the instruments

Notes on OR Data Math Function

A Notes on OR Data Math Function The ORDATA math function can accept as input either unequalized or already equalized data, and produce: RF (input): just a copy of the input waveform. Equalized: If the

Testing Power Sources for Stability

Keywords Venable, frequency response analyzer, oscillator, power source, stability testing, feedback loop, error amplifier compensation, impedance, output voltage, transfer function, gain crossover, bode

IBIS 5.0 AMI Basic Principles. Basis for existing models and existing flows

IBIS 5.0 AMI Basic Principles Basis for existing models and existing flows Walter Katz IBIS AMI October 20, 2009 Signal Integrity Software, Inc. High Speed SerDes Challenges and Simplifications Simplifications

CHARACTERIZATION and modeling of large-signal

IEEE TRANSACTIONS ON INSTRUMENTATION AND MEASUREMENT, VOL. 53, NO. 2, APRIL 2004 341 A Nonlinear Dynamic Model for Performance Analysis of Large-Signal Amplifiers in Communication Systems Domenico Mirri,

EM/Circuit Co-simulation Vratislav Sokol

EM/Circuit Co-simulation Vratislav Sokol 1 UGM 2009, Wednesday 18 th March, Darmstadt www.cst.com Agenda Motivation for EM/Circuit Co-simulation Standard versus Transient Co-simulation Standard Co-simulation

Pulsed Power Engineering Circuit Simulation

Pulsed Power Engineering Circuit Simulation January 12-16, 2009 Craig Burkhart, PhD Power Conversion Department SLAC National Accelerator Laboratory Circuit Simulation for Pulsed Power Applications Uses

Original Procedure by University of South Florida, Modified by Baylor University.

1 ELC 4384 RF/Microwave Circuits II Spring 2018 Final Design Project: Design, Simulation, and Testing of a Low-Noise Amplifier Due Thursday, April 26, 12:30 p.m. Note: This procedure has been adapted from

The wireless industry

From May 2007 High Frequency Electronics Copyright Summit Technical Media, LLC RF SiP Design Verification Flow with Quadruple LO Down Converter SiP By HeeSoo Lee and Dean Nicholson Agilent Technologies

UNIT I LINEAR WAVESHAPING

UNIT I LINEAR WAVESHAPING. High pass, low pass RC circuits, their response for sinusoidal, step, pulse, square and ramp inputs. RC network as differentiator and integrator, attenuators, its applications

Direct-Conversion I-Q Modulator Simulation by Andy Howard, Applications Engineer Agilent EEsof EDA

Direct-Conversion I-Q Modulator Simulation by Andy Howard, Applications Engineer Agilent EEsof EDA Introduction This article covers an Agilent EEsof ADS example that shows the simulation of a directconversion,

The Evolution of Waveform Relaxation for Circuit and Electromagnetic Solvers

The Evolution of Waveform Relaxation for Circuit and Electromagnetic Solvers Albert Ruehli, Missouri S&T EMC Laboratory, University of Science & Technology, Rolla, MO with contributions by Giulio Antonini,

Keysight Technologies Pulsed Antenna Measurements Using PNA Network Analyzers

Keysight Technologies Pulsed Antenna Measurements Using PNA Network Analyzers White Paper Abstract This paper presents advances in the instrumentation techniques that can be used for the measurement and

Switched-Current Circuits

Switched-urrent ircuits Outline: Synthesis and Analysis Techniques Antônio arlos Moreirão de Queiroz Signal Processing aboratory - OPPE Universidade Federal do Rio de Janeiro ntroduction. First-generation

Numerical Oscillations in EMTP-Like Programs

Session 19; Page 1/13 Spring 18 Numerical Oscillations in EMTP-Like Programs 1 Causes of Numerical Oscillations The Electromagnetic transients program and its variants all use the the trapezoidal rule

Microwave Circuits 1.1 INTRODUCTION

Microwave Circuits 1.1 INTRODUCTION The term microwave circuits means different things to different people. The prefix micro comes from the Greek fiikpog (micros) and among its various meanings has the

The prediction of non-linear waveforms in fast microwave and optotelectronic circuits through the use of a new time domain simulator.

The prediction of non-linear waveforms in fast microwave and optotelectronic circuits through the use of a new time domain simulator. by Dr Joseph A. Barnard and Michael Taylor Barnard Microsystems Limited

Using Sonnet EM Analysis with Cadence Virtuoso in RFIC Design. Sonnet Application Note: SAN-201B July 2011

Using Sonnet EM Analysis with Cadence Virtuoso in RFIC Design Sonnet Application Note: SAN-201B July 2011 Description of Sonnet Suites Professional Sonnet Suites Professional is an industry leading full-wave

VCO Design Project ECE218B Winter 2011

VCO Design Project ECE218B Winter 2011 Report due 2/18/2011 VCO DESIGN GOALS. Design, build, and test a voltage-controlled oscillator (VCO). 1. Design VCO for highest center frequency (< 400 MHz). 2. At

EEM478-DSPHARDWARE. WEEK12:FIR & IIR Filter Design

EEM478-DSPHARDWARE WEEK12:FIR & IIR Filter Design PART-I : Filter Design/Realization Step-1 : define filter specs (pass-band, stop-band, optimization criterion, ) Step-2 : derive optimal transfer function

SAMPLING WITH AUTOMATIC GAIN CONTROL

SAMPLING WITH AUTOMATIC GAIN CONTROL Impulse Sampler Interpolation Iterative Optimization Automatic Gain Control Tracking Example: Time-Varying Fade idealized system Software Receiver Design Johnson/Sethares/Klein

LINEAR MODELING OF A SELF-OSCILLATING PWM CONTROL LOOP

Carl Sawtell June 2012 LINEAR MODELING OF A SELF-OSCILLATING PWM CONTROL LOOP There are well established methods of creating linearized versions of PWM control loops to analyze stability and to create

A User s Guide to Envelope Following Analysis

Application Note A User s Guide to Envelope Following Analysis The procedures described in this application note are deliberately broad and generic. Requirements for your specific design may dictate procedures

Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL

Mor M. Peretz Power Electronics Laboratory Department of Electrical and Computer Engineering Ben-Gurion University of the Negev, ISRAEL [1] PSpice A/D simulation program allows to analyze electrical circuits

Measurements 2: Network Analysis

Measurements 2: Network Analysis Fritz Caspers CAS, Aarhus, June 2010 Contents Scalar network analysis Vector network analysis Early concepts Modern instrumentation Calibration methods Time domain (synthetic

Application of Fourier Transform in Signal Processing

1 Application of Fourier Transform in Signal Processing Lina Sun,Derong You,Daoyun Qi Information Engineering College, Yantai University of Technology, Shandong, China Abstract: Fourier transform is a

Lab 10: Oscillators (version 1.1)

Lab 10: Oscillators (version 1.1) WARNING: Use electrical test equipment with care! Always double-check connections before applying power. Look for short circuits, which can quickly destroy expensive equipment.

Laboratory Assignment 5 Amplitude Modulation

Laboratory Assignment 5 Amplitude Modulation PURPOSE In this assignment, you will explore the use of digital computers for the analysis, design, synthesis, and simulation of an amplitude modulation (AM)

TRANSFORMS / WAVELETS

RANSFORMS / WAVELES ransform Analysis Signal processing using a transform analysis for calculations is a technique used to simplify or accelerate problem solution. For example, instead of dividing two

A Simplified Extension of X-parameters to Describe Memory Effects for Wideband Modulated Signals

Jan Verspecht bvba Mechelstraat 17 B-1745 Opwijk Belgium email: contact@janverspecht.com web: http://www.janverspecht.com A Simplified Extension of X-parameters to Describe Memory Effects for Wideband

Harmonic Balance Simulation

Harmonic Balance Simulation September 2004 Notice The information contained in this document is subject to change without notice. Agilent Technologies makes no warranty of any kind with regard to this

EE320L Electronics I. Laboratory. Laboratory Exercise #2. Basic Op-Amp Circuits. Angsuman Roy. Department of Electrical and Computer Engineering

EE320L Electronics I Laboratory Laboratory Exercise #2 Basic Op-Amp Circuits By Angsuman Roy Department of Electrical and Computer Engineering University of Nevada, Las Vegas Objective: The purpose of

Modeling the Effect of Wire Resistance in Deep Submicron Coupled Interconnects for Accurate Crosstalk Based Net Sorting

Modeling the Effect of Wire Resistance in Deep Submicron Coupled Interconnects for Accurate Crosstalk Based Net Sorting C. Guardiani, C. Forzan, B. Franzini, D. Pandini Adanced Research, Central R&D, DAIS,

Module 3 : Sampling and Reconstruction Problem Set 3

Module 3 : Sampling and Reconstruction Problem Set 3 Problem 1 Shown in figure below is a system in which the sampling signal is an impulse train with alternating sign. The sampling signal p(t), the Fourier

CHAPTER 6 DIGITAL CIRCUIT DESIGN USING SINGLE ELECTRON TRANSISTOR LOGIC

94 CHAPTER 6 DIGITAL CIRCUIT DESIGN USING SINGLE ELECTRON TRANSISTOR LOGIC 6.1 INTRODUCTION The semiconductor digital circuits began with the Resistor Diode Logic (RDL) which was smaller in size, faster

if the conductance is set to zero, the equation can be written as following t 2 (4)

1 ECEN 720 High-Speed Links: Circuits and Systems Lab1 - Transmission Lines Objective To learn about transmission lines and time-domain reflectometer (TDR). Introduction Wires are used to transmit clocks

R. W. Erickson. Department of Electrical, Computer, and Energy Engineering University of Colorado, Boulder

R. W. Erickson Department of Electrical, Computer, and Energy Engineering University of Colorado, Boulder pn junction! Junction diode consisting of! p-doped silicon! n-doped silicon! A p-n junction where

Principles of Analog In-Circuit Testing By Anthony J. Suto, Teradyne, December 2012 In-circuit test (ICT) has been instrumental in identifying manufacturing process defects and component defects on countless

Biomedical Signals. Signals and Images in Medicine Dr Nabeel Anwar

Biomedical Signals Signals and Images in Medicine Dr Nabeel Anwar Noise Removal: Time Domain Techniques 1. Synchronized Averaging (covered in lecture 1) 2. Moving Average Filters (today s topic) 3. Derivative

Linear networks analysis

Linear networks analysis For microwave linear networks analysis is performed in frequency domain. The analysis is based on the evaluation of the scattering matrix of the n port network From S matrix all

I1 19u 5V R11 1MEG IDC Q7 Q2N3904 Q2N3904. Figure 3.1 A scaled down 741 op amp used in this lab

Lab 3: 74 Op amp Purpose: The purpose of this laboratory is to become familiar with a two stage operational amplifier (op amp). Students will analyze the circuit manually and compare the results with SPICE.

Direct Harmonic Analysis of the Voltage Source Converter

1034 IEEE TRANSACTIONS ON POWER DELIVERY, VOL. 18, NO. 3, JULY 2003 Direct Harmonic Analysis of the Voltage Source Converter Peter W. Lehn, Member, IEEE Abstract An analytic technique is presented for

Basic Electronics Learning by doing Prof. T.S. Natarajan Department of Physics Indian Institute of Technology, Madras

Basic Electronics Learning by doing Prof. T.S. Natarajan Department of Physics Indian Institute of Technology, Madras Lecture 26 Mathematical operations Hello everybody! In our series of lectures on basic

FDTD SPICE Analysis of High-Speed Cells in Silicon Integrated Circuits

FDTD Analysis of High-Speed Cells in Silicon Integrated Circuits Neven Orhanovic and Norio Matsui Applied Simulation Technology Gateway Place, Suite 8 San Jose, CA 9 {neven, matsui}@apsimtech.com Abstract

print close Related Low-Cost UWB Source Low-Cost Mixers Build On LTCC Reliability LTCC Launches Miniature, Wideband, Low-Cost Mixers

print close Design A Simple, Low-Cost UWB Source Microwaves and RF Yeap Yean Wei Fri, 2006-12-15 (All day) Using an inexpensive commercial step recovery diode (SRD) and a handful of passive circuit elements,

A 2.6GHz/5.2GHz CMOS Voltage-Controlled Oscillator*

WP 23.6 A 2.6GHz/5.2GHz CMOS Voltage-Controlled Oscillator* Christopher Lam, Behzad Razavi University of California, Los Angeles, CA New wireless local area network (WLAN) standards have recently emerged

THE TREND toward implementing systems with low

724 IEEE JOURNAL OF SOLID-STATE CIRCUITS, VOL. 30, NO. 7, JULY 1995 Design of a 100-MHz 10-mW 3-V Sample-and-Hold Amplifier in Digital Bipolar Technology Behzad Razavi, Member, IEEE Abstract This paper

Figure Main frame of IMNLab.

IMNLab Tutorial This Tutorial guides the user to go through the design procedure of a wideband impedance match network for a real circuit by using IMNLab. Wideband gain block TQP3M97 evaluation kit from

Characterization Methodology for High Density Microwave Fixtures. Dr. Brock J. LaMeres, Montana State University

DesignCon 2008 Characterization Methodology for High Density Microwave Fixtures Dr. Brock J. LaMeres, Montana State University lameres@ece.montana.edu Brent Holcombe, Probing Technology, Inc brent.holcombe@probingtechnology.com

NEW WIRELESS applications are emerging where

IEEE JOURNAL OF SOLID-STATE CIRCUITS, VOL. 39, NO. 4, APRIL 2004 709 A Multiply-by-3 Coupled-Ring Oscillator for Low-Power Frequency Synthesis Shwetabh Verma, Member, IEEE, Junfeng Xu, and Thomas H. Lee,

Karadeniz Technical University Department of Electrical and Electronics Engineering Trabzon, Turkey

Karadeniz Technical University Department of Electrical and Electronics Engineering 61080 Trabzon, Turkey Chapter 3-2- 1 Modelling and Representation of Physical Systems 3.1. Electrical Systems Bu ders

Chapter 9. Digital Communication Through Band-Limited Channels. Muris Sarajlic

Chapter 9 Digital Communication Through Band-Limited Channels Muris Sarajlic Band limited channels (9.1) Analysis in previous chapters considered the channel bandwidth to be unbounded All physical channels

A SIGNAL DRIVEN LARGE MOS-CAPACITOR CIRCUIT SIMULATOR

A SIGNAL DRIVEN LARGE MOS-CAPACITOR CIRCUIT SIMULATOR Janusz A. Starzyk and Ying-Wei Jan Electrical Engineering and Computer Science, Ohio University, Athens Ohio, 45701 A designated contact person Prof.

EE390 Final Exam Fall Term 2002 Friday, December 13, 2002

Name Page 1 of 11 EE390 Final Exam Fall Term 2002 Friday, December 13, 2002 Notes 1. This is a 2 hour exam, starting at 9:00 am and ending at 11:00 am. The exam is worth a total of 50 marks, broken down

Department of Mechanical and Aerospace Engineering. MAE334 - Introduction to Instrumentation and Computers. Final Examination.

Name: Number: Department of Mechanical and Aerospace Engineering MAE334 - Introduction to Instrumentation and Computers Final Examination December 12, 2002 Closed Book and Notes 1. Be sure to fill in your

Methods and Approaches for RF Circuit Simulation And Electromagnetic Modelling

Methods and Approaches for RF Circuit Simulation And Electromagnetic Modelling T.A.M. Kevenaar 1, E.J.W. ter Maten 1, H.H.J. Janssen 1, S. Onneweer 2 1 Philips Research, Eindhoven, The Netherlands 2 Philips

ICI Mitigation for Mobile OFDM with Application to DVB-H

ICI Mitigation for Mobile OFDM with Application to DVB-H Outline Background and Motivation Coherent Mobile OFDM Detection DVB-H System Description Hybrid Frequency/Time-Domain Channel Estimation Conclusions

Thank you Carmina. Welcome all to our presentation of Direct Filter Synthesis for Customized Response

Thank you Carmina. Welcome all to our presentation of Direct Filter Synthesis for Customized Response 1 This is just a brief review of our agenda, first we will review the Functions and types of filters

RF Board Design for Next Generation Wireless Systems

RF Board Design for Next Generation Wireless Systems Page 1 Introduction Purpose: Provide basic background on emerging WiMax standard Introduce a new tool for Genesys that will aide in the design and verification

2.2 INTERCONNECTS AND TRANSMISSION LINE MODELS

CHAPTER 2 MODELING OF SELF-HEATING IN IC INTERCONNECTS AND INVESTIGATION ON THE IMPACT ON INTERMODULATION DISTORTION 2.1 CONCEPT OF SELF-HEATING As the frequency of operation increases, especially in the

Fourier Theory & Practice, Part I: Theory (HP Product Note )

Fourier Theory & Practice, Part I: Theory (HP Product Note 54600-4) By: Robert Witte Hewlett-Packard Co. Introduction: This product note provides a brief review of Fourier theory, especially the unique

CHAPTER 9 Sinusoidal Steady-State Analysis 9.1 The Sinusoidal Source A sinusoidal voltage source (independent or dependent) produces a voltage that varies sinusoidally with time. A sinusoidal current source

332:223 Principles of Electrical Engineering I Laboratory Experiment #2 Title: Function Generators and Oscilloscopes Suggested Equipment:

RUTGERS UNIVERSITY The State University of New Jersey School of Engineering Department Of Electrical and Computer Engineering 332:223 Principles of Electrical Engineering I Laboratory Experiment #2 Title: