Laboratory 3. EE 342 (VLSI Circuit Design) - Using Spectre netlist and Calculator for simulation
|
|
- Kenneth Hood
- 6 years ago
- Views:
Transcription
1 EE 342 (VLSI Circuit Design) Laboratory 3 - Using Spectre netlist and Calculator for simulation By Mulong Li,
2 Background knowledge Spectre: is a SPICE-class circuit simulator. It provides the basic SPICE analyses and component models. Spectre comes in enhanced versions that also support RF simulation (SpectreRF) and mixed-signal simulation (AMS Designer). It was developed at Cadence Design Systems, and is currently a leading circuit simulator, competing with HSPICE and several others Netlist: describes the structure of circuits and subcircuits by listing components, the nodes that the components are connected to, the parameter values that are used to customize the components, and the analyses that you want to run on the circuit. Common Linux commands: Below are some of the most common Linux commands that you may need to use in this tutorial. - cd /directorypath: Change to directory o. indicates the current directory,.. indicates the parent directory, ~ indicates the user s home directory. For example, cd.. means move to the parent directory - pwd: Show the path of the current directory - ls: List directory contents - cp source destination: Copy files and directories - mv source destination: Rename or move file(s) or directories - mkdir directory: Create a new directory - rm filename: Permanently remove file(s) and/or directories. - gedit filename [&]: Open a file with gedit text editor. If file name does not exist, create a new one. Add & to run the job in background, so that you can run other commands using the current terminal window when the job is running 2
3 1 Netlist and Spectre syntax In this tutorial, we will run the simulation by writing a netlist in Spectre. Spectre syntax is different from SPICE. In this part, we are going to create a simple netlist file using Spectre syntax. 1.1 Login the Linux machine and open a new terminal window. 1.2 Create a new directory a) In the terminal window, create a new directory for this course and this lab in your cabinet: $ mkdir ~/cabinet/cme342/cadence_netlist b) Go to the newly created directory. $ cd ~/cabinet/cme342/cadence_netlist/ And source the toolkit again: $ source /CMC/scripts/kit.tsmc180nm.5.2.csh c) We will then create the netlist file and run simulation under this directory. d) In the current directory, create a new text file called example_ckt.scs. $ gedit example_ckt.scs e) Read carefully and try to understand the following codes, and then copy them into the example_ckt.scs file: //Design cell name: example_ckt simulator lang=spectre //use Spectre syntax global 0 vdd! //set global signals //include model library include "/usr/local/bin/cadence_lib/models/spectre/icfspectre.init" 3
4 //vdd! voltage is 1.8V V0 (vdd! 0) vsource dc=1.8 type=dc //V1 is a pulse shape voltage source V1 (net_a 0) vsource type=pulse val0=0 val1=1.8 period=2n delay=1n width=1n //M0 (d g s b) is a 500nm*180nm PMOS //as, ad: source/drain area; ps, pd: s/d perimeter; nrs, nrd: # of squares in s/d M0 (net_out vdd! vdd! vdd!) pch w=500n l=180.00n as=0.48u*(500n) \ ad=0.48u*(500n) ps=0.96u+2*(500n) pd=0.96u+2*(500n) \ nrd=0.27u/(500n ) nrs=0.27u/(500n) m=1 region=triode M1 (net_out net_a vdd! vdd!) pch w=500n l=180.00n as=0.48u*(500n) \ ad=0.48u*(500n) ps=0.96u+2*(500n) pd=0.96u+2*(500n) \ nrd=0.27u/(500n) nrs=0.27u/(500n) m=1 region=triode M2 (net_out net_a net1 0) nch w=500n l=180.00n as=0.48u*(500n) \ ad=0.48u*(500n) ps=0.96u+2*(500n) pd=0.96u+2*(500n) \ nrd=0.27u/(500n) nrs=0.27u/(500n) m=1 region=triode M3 (net1 vdd! 0 0) nch w=500n l=180.00n as=0.48u*(500n) ad=0.48u*(500n) \ ps=0.96u+2*(500n) pd=0.96u+2*(500n) nrd=0.27u/(500n) \ nrs=0.27u/(500n) m=1 region=triode //run transient analysis, set the stop time to 5ns tran tran stop=5n write="spectre.ic" writefinal="spectre.fc" \ annotate=status maxiters=5 //save all signals saveoptions options save=allpub f) Save the file. 4
5 1.3 Now with the circuit structure in the netlist, we can start doing some simulation. a) In the terminal, start the Spectre simulation with the following command: (-f psfascii specifies the output data format) $ spectre example_ckt.scs f psfascii b) Then you will see the transient analysis running. c) When the terminal shows spectre completes with 0 errors, X warnings, and 0 notices, the simulation is done. Now you ll see a new directory example_ckt.raw under your cadence_netlist directory. All the simulated signals are saved in it. 1.4 Now we will use Results Browser to view our simulation results. a) Go up to your home directory ($ cd ~), and start the Cadence program ($ cadence). b) In the icfb window, select Tool -> Analog Environment -> Results Browser. Open example_ckt.raw -> tran-tran, you ll see a list of signals in the example circuit, similar to Figure 1-1. Figure 1.1 c) Choose the signals you want to see, and click Plot signal. A graph window will pop out as in Figure
6 Figure 1.2 Exercise A: Design a 3-input NOR gate in netlist, with transistor widths chosen to achieve equal rise and fall resistance as a unit inverter (assume a unit inverter has size: N 500nm, P 1um). Inputs are net_a = net_b = 0 and net_c = 500MHz pulse, output is net_out. Measure the net_c to net_out delay. 6
7 2 Virtuoso Tools and Calculator Now we will use Virtuoso tools to build circuits and run simulations in a more straightforward way. Let s start by making a simple D-latch. 2.1 Create schematic a) In icfb window, open Library Manager. Select library abc123 (your NSID), and create a new schematic view with cell name D_latch (never use - when naming libraries or cells, the tool may not recognise it). b) Add nfets and pfets to the schematic. Also we need to add supplies vdd and gnd from the library analoglib. Press q to change the size of the transistors so that the width of NMOS and PMOS are 500nm and 1um respectively, while the lengths are both 180nm. The schematic should now look like this: Figure 2.1 7
8 c) Now connect all the instances.as in Figure 2-2. Don't forget to connect bulk terminals of pfets to vdd and that of nfets to gnd by adding wire names vdd! and gnd!. Figure 2.2 d) Add 3 input pins: D_in, Clock and Clock_bar to the left, and 2 output pins: Q_out and Q_bar on the right. 8
9 e) Add wire corresponding names to connect to all the pins. Remember to click Check and save to see if there s any error! f) Create a symbol view as well. Figure Schematic simulations a) After the schematic and symbol view are created, we need to create a testbench cell and instance the latch within it to test its functionality. b) First, select library abc123 in the Library Manager, and create a new Schematic cell view called D_latch_tb. c) Add instances of vpulse and vdc from analoglib to D_latch_tb, as well as vdd and gnd. Also add the symbol of D_latch created in the previous step. Add 2 output pins Q and Qbar. Connect all the components as in Figure
10 Figure 2.4 d) Modify the properties of the added components. For vpulse to D_in Figure
11 For vpulse to Clock_bar For vpulse to Clock Figure 2.6 For vdc Figure 2.7 Figure 2.8 e) Keep all the other parameters default. Check and save. 11
12 2.3 Waveform results a) Click Tools -> Analog Environment to open ADE window. b) Go to Setup -> Model libraries. Add Model Library File /usr/local/bin/cadence_lib/models/spectre/icfspectre.init. c) Go to Outputs -> Save All -> Select power signals to output (pwr), check total. This step is needed for estimating power later on. d) Go to Analyses -> choose, choose tran (transient analyses) and set stop time to 500ns. Long stop time is needed for more accurate average power estimation. Click OK. e) Select all the inputs and outputs of the D-latch to be plotted. Press Esc after you have selected all the signals you need, you ll see the signals now in ADE. f) Click to start simulation. It will take up to several minutes to do compiling work for the first time. When the simulation is done, a plot will pop up showing the simulation results. (You can check the error information in icfb window if any) Figure
13 g) Click Strip Chart Mode to separate signals. Check if your D-latch works properly. 2.4 Calculator a) Delay 1). Click Tools -> Calculator to open the Calculator. Make sure vt under tab tran is selected. Figure ). We will now use the delay function to measure the D to Q delay of the Latch. Click on delay in the function panel, and you will see the delay function window as in Figure Adjust the window to see all the options. Figure
14 3). Click in Signal1 field, then switch to the Schematic window, and click on the D_in (input) signal. You will notice that the Signal1 filed is now replaced by the vt signal of the wire you click on. 4). Repeat the last step to replace Signal2 with Q (output) signal. 5). Set Threshold Value to 0.9 and the other parameters default as show in Figure Set Edge Type to both rising or both falling, so as to measure rising or falling edge delay. 6). Click Apply, then click plot. The delay should be evaluated to around 25ps. b) Frequency 1). Calculate signal frequency with the frequency function. 2). Click on clk (clock) signal in the schematic, then go back to Calculator and click on frequency function. Click Plot, the frequency should be evaluated to about 100MHz. c) Power Consumption 1). In the Graph window, go to Tools -> Results Browser. 2). Select tran-tran, and double click on \:pwr. The Graph window will pop up. Figure
15 3). Go to Calculator, click average in the function panel, and click plot, you ll get an average power consumption of 5.1 uw. 4). Select wave in Selection choices, switch to Graph window and click on the dynamic power waveform. Switch back to Calculator and choose function ymax. Click Plot, and you ll obtain the maximum power consumption of 0.37 mw. Exercise B: 1. Design a D latch with an ENABLE signal using NAND gates (P 1um, N 1um). Draw the schematic, build a test bench to test its functionality, and measure its D to Q delay and average/maximum power consumption using Calculator function. 2. Design a 1.2 GHz ring oscillator using the following inverter size: P 1um, N 500nm. Use Calculator to verify its frequency. (Hint: set Initial Condition to make it oscillate ) Report: 1. Exercise A: Netlist of your NOR gate 2. Exercise B1: Schematic of D latch and its test bench 3. Exercise B2: Schematic of ring oscillator 4. Waveforms of all the simulation along with your Calculator results Instruction: How to print schematic with a white background? (If you want to save some ink) Method 1: Invert colors in Paint. Or in Microsoft Word 2010, click on your figure, go to Picture tools -> Format -> Color -> Set Transparent color -> click on the black background. 15
16 Method 2: This method will change all the schematics and layouts background color in your current cadence session. Type the following command in your terminal: echo "Opus.editorBackground: white" xrdb merge You have to restart cadence to make it work. To change back to black background: echo "Opus.editorBackground: black" xrdb -merge 16
Cadence Tutorial. Introduction to Cadence 0.18um, Implementation and Simulation of an inverter. A. Moradi, A. Miled et M. Sawan
Cadence Tutorial Introduction to Cadence 0.18um, Implementation and Simulation of an inverter A. Moradi, A. Miled et M. Sawan Section 1: Introduction to Cadence You will see how to create a new library
More informationIntroduction to laboratory exercises in Digital IC Design.
Introduction to laboratory exercises in Digital IC Design. A digital ASIC typically consists of four parts: Controller, datapath, memory, and I/O. The digital ASIC below, which is an FFT/IFFT co-processor,
More informationCS755 CAD TOOL TUTORIAL
CS755 CAD TOOL TUTORIAL CREATING SCHEMATIC IN CADENCE Shi-Ting Zhou shi-ting@cs.wisc.edu After you have figured out what you want to design, and drafted some pictures and diagrams, it s time to input schematics
More informationEE115C Digital Electronic Circuits. Tutorial 2: Hierarchical Schematic and Simulation
EE115C Digital Electronic Circuits Tutorial 2: Hierarchical Schematic and Simulation The objectives are to become familiar with Virtuoso schematic editor, learn how to create the symbol view of basic primitives,
More informationCPE/EE 427, CPE 527, VLSI Design I: Tutorial #2, Schematic Capture, DC Analysis, Transient Analysis (Inverter, NAND2)
CPE/EE 427, CPE 527, VLSI Design I: Tutorial #2, Schematic Capture, DC Analysis, Transient Analysis (Inverter, NAND2) Joel Wilder, Aleksandar Milenkovic, ECE Dept., The University of Alabama in Huntsville
More informationCadence Schematic Tutorial. EEE5320/EEE4306 Fall 2015 University of Florida ECE
Cadence Schematic Tutorial EEE5320/EEE4306 Fall 2015 University of Florida ECE 1 Remote access You may access the Linux server directly from the NEB Computer Lab using your GatorLink username and password.
More informationCadence Tutorial: Schematic Entry and Circuit Simulation of a CMOS Inverter
Cadence Tutorial: Schematic Entry and Circuit Simulation of a CMOS Inverter Introduction This tutorial describes the steps involved in the design and simulation of a CMOS inverter using the Cadence Virtuoso
More informationThe following is a procedure for extracting a layout, doing a layout vs. schematic check, and then simulating the extracted layout with Cadence.
The following is a procedure for extracting a layout, doing a layout vs. schematic check, and then simulating the extracted layout with Cadence. (This might not be the best way, but it works!) 1) Realize
More informationS Exercise 1C Testing the Ring Oscillator
S-87.3148 Exercise 1C Testing the Ring Oscillator Aalto University School of Electrical Engineering Department of Micro- and Nanosciences (ECDL) 10.9.2014 1 1 Building the test bench In this exercise,
More informationEE 330 Spring Laboratory 2: Basic Boolean Circuits
EE 330 Spring 2013 Laboratory 2: Basic Boolean Circuits Objective: The objective of this experiment is to investigate methods for evaluating the performance of Boolean circuits. Emphasis will be placed
More informationCadence Tutorial A: Schematic Entry and Functional Simulation Created for the MSU VLSI program by Professor A. Mason and the AMSaC lab group.
Cadence Tutorial A: Schematic Entry and Functional Simulation Created for the MSU VLSI program by Professor A. Mason and the AMSaC lab group. Revision Notes: Jan. 2006 Updated for use with spectre simulator
More informationCadence Tutorial A: Schematic Entry and Functional Simulation Created for the MSU VLSI program by Andrew Mason and the AMSaC lab group.
Cadence Tutorial A: Schematic Entry and Functional Simulation Created for the MSU VLSI program by Andrew Mason and the AMSaC lab group. Revision Notes: Aug. 2003 update and edit A. Mason add intro/revision/contents
More informationThe original document link is
Tutorial:Analog Artist with HSPICE The original document link is http://www.eda.ncsu.edu/wiki/tutorial:analog_artist_with_hspice This tutorial will introduce you to the Cadence Environment: specifically
More informationDOWNLOAD PDF CADENCE WAVEFORM CALCULATOR USER GUIDE
Chapter 1 : CSE / Cadence Tutorial The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems
More informationESE 570 Cadence Lab Assignment 2: Introduction to Spectre, Manual Layout Drawing and Post Layout Simulation (PLS)
ESE 570 Cadence Lab Assignment 2: Introduction to Spectre, Manual Layout Drawing and Post Layout Simulation (PLS) Objective Part A: To become acquainted with Spectre (or HSpice) by simulating an inverter,
More informationCadence Tutorial C: Simulating DC and Timing Characteristics 1
Cadence Tutorial C: Simulating DC and Timing Characteristics Created for the MSU VLSI program by Professor A. Mason and the AMSaC lab group Last updated by Patrick O Hara SS15 Document Contents Introduction
More informationLab 2: Functional Simulation Using. Affirma Analog Simulator
Lab 2: Functional Simulation Using Affirma Analog Simulator This Lab will go over: 1. Creating a test bench 2. Simulation in Spectre Spice using the Analog Design environment 1. Creating a test bench:
More informationEE 330 Spring 2018 Laboratory 2: Basic Boolean Circuits
EE 330 Spring 2018 Laboratory 2: Basic Boolean Circuits Contents Objective:... 2 Part 1: Introduction... 2 Part 2 Simulation of a CMOS Inverter... 3 Part 2.1 Attaching technology information... 3 Part
More informationCadence Virtuoso Schematic Design and Circuit Simulation Tutorial
Cadence Virtuoso Schematic Design and Circuit Simulation Tutorial Introduction This tutorial is an introduction to schematic capture and circuit simulation for ENGN1600 using Cadence Virtuoso. These courses
More informationEECE 285 VLSI Design. Cadence Tutorial EECE 285 VLSI. By: Kevin Dick Co-author: Jeff Kauppila Co-author: Dr. Arthur Witulski
Cadence Tutorial EECE 285 VLSI By: Kevin Dick Co-author: Jeff Kauppila Co-author: Dr. Arthur Witulski 1 Table of Contents Purpose of Cadence 1) The Purpose of Cadence pg. 4 Linux 1) The Purpose of Linux
More informationTutorial on getting started in Cadence. Advanced Analog Circuits Spring 2015 Instructor: Prof. Harish Krishnaswamy TA: Jahnavi Sharma
Tutorial on getting started in Cadence Advanced Analog Circuits Spring 2015 Instructor: Prof. Harish Krishnaswamy TA: Jahnavi Sharma Getting Started Start Cadence from the terminal by using the command
More informationSimulation with Verilog-XL
Simulation with Verilog-XL Adapted from Princeton Cadence Page (http://www.ee.princeton.edu/~cadence/usr/verilog.html) Until now, we have been using the Analog Environment to do simulations. This simulator
More informationEE 330 Spring 2018 Lab 1: Cadence Custom IC design tools Setup, Schematic capture and simulation
EE 330 Spring 2018 Lab 1: Cadence Custom IC design tools Setup, Schematic capture and simulation Table of Contents Objective... 2 1. Setup... 2 Set Bash Shell for the account... 2 2. Starting Cadence Custom
More informationCMOS Design Lab Manual
CMOS Design Lab Manual Developed By University Program Team CoreEl Technologies (I) Pvt. Ltd. 1 Objective Objective of this lab is to learn the Mentor Graphics HEP2 tools as well learn the flow of the
More informationEE 330 Fall 2017 Lab 1: Cadence Custom IC design tools - Setup, Schematic capture and simulation
EE 330 Fall 2017 Lab 1: Cadence Custom IC design tools - Setup, Schematic capture and simulation Table of Contents Objective... 2 1. Setup... 2 Set Bash Shell for the account... 2 2. Starting Cadence Custom
More informationCADENCE SETUP. ECE4430-Analog IC Design
CADENCE SETUP This short tutorial shows how to configure Cadence to use the NCSU Cadence Design Kit (CDK) with access to the ON Semiconductor C5 0.5-µm and the TSMC 0.35-µm CMOS processes libraries. In
More informationECE 546 HOMEWORK No 10 Due Thursday, April 19, yes last
ECE 546 HOMEWORK No 10 Due Thursday, April 19, 2018 In this homework you will extract the pulse response of the given channel, extract the decision feedback equalization (DFE) coefficients to equalize
More informationEE4111 Advanced Analog Electronics Design. Spring 2009 Experiment #4 April 6 ~ April 17
EE4111 Advanced Analog Electronics Design Spring 2009 Experiment #4 April 6 ~ April 17 Setup Cadence in VLSI Lab 1) Copy files $ cp r /home/grads/ee4111ta ~/ 2) Edit your.cshrc file -- Include the following
More informationLab 2. Standard Cell layout.
Lab 2. Standard Cell layout. The purpose of this lab is to demonstrate CMOS-standard cell design. Use the lab instructions and the cadence manual (http://www.es.lth.se/ugradcourses/cadsys/cadence.html)
More informationAMS 0.18 µm PDK Setup and Cadence Tutorial Contributors
AMS 0.18 µm PDK Setup and Cadence Tutorial Contributors Muhammad Ahmed, Sita Asar, and Ayman Fayed, Power Management Research Lab, https://pmrl.osu.edu, Department of Electrical and Computer Engineering,
More informationFigure 1: ADE Test Editor
Due to some issues that ADE GXL simulation environment has (probably because of inappropriate setup), we will run simulations in the ADE L design environment, which includes all the necessary tools that
More informationLogic synthesis and Place and Route Tutorial Page 1
Logic synthesis and Place and Route Tutorial Page 1 Standard Cell ASIC Design flow: A designer uses predesigned logic cells such as AND gate, NOR gate, etc. These gates are called Standard Cells. The advantage
More informationINTRODUCTION TO MENTOR GRAPHICS DESIGN TOOLS
INTRODUCTION TO MENTOR GRAPHICS DESIGN TOOLS 1. RUNNING MENTOR GRAPHICS Erdem S. Erdogan 09.13.2006 Note: These commands can be run remotely via ssh to one of the DSIL machines. If running remotely, ignore
More informationECE 331: Electronics Principles I Fall 2014
ECE 331: Electronics Principles I Fall 2014 Lab #0: Introduction to Computer Modeling and Laboratory Measurements Report due at your registered lab period on the week of Sept. 8-12 Week 1 Accessing Linux
More informationCadence Tutorial D: Using Design Variables and Parametric Analysis Document Contents Introduction Using Design Variables Apply Apply
Cadence Tutorial D: Using Design Variables and Parametric Analysis Created for the MSU VLSI program by Casey Wallace Last Updated by: Patrick O Hara SS15 Document Contents Introduction Using Design Variables
More informationECE471/571 Energy Efficient VLSI Design Project 2 Cadence Setup and Creation of an Inverter Due Date 11:30 am on Friday, February 2 nd, 2018
ECE471/571 Energy Efficient VLSI Design Project 2 Cadence Setup and Creation of an Inverter Due Date 11:30 am on Friday, February 2 nd, 2018 Introduction This project will first walk you through the setup
More informationRevision Notes: July2004 Generate tutorial for single transistor analysis. Based on existing schematic entry tutorial developed for ECE410
Cadence Analog Tutorial 1: Schematic Entry and Transistor Characterization Created for the MSU VLSI program by Professor A. Mason and the AMSaC lab group. Revision Notes: July2004 Generate tutorial for
More informationLab 1: An Introduction to Cadence
GIF-4201/GEL-7016 (Micro-électronique) Lab 1: An Introduction to Cadence Schematic, simulation and layout Gabriel Gagnon-Turcotte, Mehdi Noormohammadi Khiarak and Benoit Gosselin Department of Electrical
More informationProfessor Muller Fall 2016 Sameet Ramakrishnan Eric Chang Adapted from prior EE140 and EE141 labs. EE 140/240A Lab 0 Full IC Design Flow
Professor Muller Fall 2016 Sameet Ramakrishnan Eric Chang Adapted from prior EE140 and EE141 labs EE 140/240A Lab 0 Full IC Design Flow In this lab, you will walk through the full process an analog designer
More informationECE471/571 Energy Ecient VLSI Design
ECE471/571 Energy Ecient VLSI Design Project 2 Cadence Setup and Creation of an Inverter Due Date 11:30pm on Friday, January 30 th 2015 Introduction This project will rst walk you through the setup for
More informationSelect the technology library: NCSU_TechLib_ami06, then press OK.
ECE 126 Inverter Tutorial: Schematic & Symbol Creation Created for GWU by Anis Nurashikin Nordin & Thomas Farmer Tutorial adapted from: http://www.ee.ttu.edu/ee/cadence/commondirectory/final%20tutorials/digitalcircuitsimulationusingvirtuoso.doc
More informationUNIVERSITY OF WATERLOO
UNIVERSITY OF WATERLOO UW ASIC DESIGN TEAM: Cadence Tutorial Description: Part I: Layout & DRC of a CMOS inverter. Part II: Extraction & LVS of a CMOS inverter. Part III: Post-Layout Simulation. The Cadence
More informationCS/EE 5720/6720 Analog IC Design Tutorial for Schematic Design and Analysis using Spectre
CS/EE 5720/6720 Analog IC Design Tutorial for Schematic Design and Analysis using Spectre Introduction to Cadence EDA: The Cadence toolset is a complete microchip EDA (Electronic Design Automation) system,
More informationEEC 118 Spring 2011 Lab #5 Manchester Carry-Chain Adder
EEC 118 Spring 2011 Lab #5 Manchester Carry-Chain Adder Rajeevan Amirtharajah Dept. of Electrical and Computer Engineering University of California, Davis Issued: May 9, 2011 Due: May 20, 2011, 5 PM in
More informationLTSPICE MANUAL. For Teaching Module EE4415 ZHENG HAUN QUN. December 2016
LTSPICE MANUAL For Teaching Module EE4415 ZHENG HAUN QUN December 2016 DEPARTMENT OF ELECTRICAL AND COMPUTER ENGINNERING NATIONAL UNIVERSITY OF SINGAPORE Contents 1. Introduction... 2 1.1 Installation...
More informationCadence Tutorial 2: Layout, DRC/LVS and Circuit Simulation with Extracted Parasitics
Cadence Tutorial 2: Layout, DRC/LVS and Circuit Simulation with Extracted Parasitics Introduction This tutorial describes how to generate a mask layout in the Cadence Virtuoso Layout Editor. Use of DIVA
More informationAmplifier Simulation Tutorial. Design Kit: Cadence 0.18μm CMOS PDK (gpdk180) (Cadence Version 6.1.5)
Amplifier Simulation Tutorial Design Kit: Cadence 0.18μm CMOS PDK (gpdk180) (Cadence Version 6.1.5) Yongsuk Choi, Marvin Onabajo This tutorial provides a quick introduction to the use of Cadence tools
More informationVirtuoso Schematic Composer
is a schematic design tool from Cadence. In this tutorial you will learn how to put electrical components, make wire connections, insert pins and check for connection error. Start Cadence Custom IC Design
More informationESE570 Spring University of Pennsylvania Department of Electrical and System Engineering Digital Integrated Cicruits AND VLSI Fundamentals
University of Pennsylvania Department of Electrical and System Engineering Digital Integrated Cicruits AND VLSI Fundamentals ESE570, Spring 2019 HW5: Delay and Layout Sunday, February 17th Due: Friday,
More informationEE 471: Transport Phenomena in Solid State Devices
EE 471: Transport Phenomena in Solid State Devices HW7 Due: 4/17/18 For this homework, you will download a free PC version of the industry standard SPICE circuit simulator called LTspice, provided by Linear
More informationLab 1: Cadence Custom IC design tools- Setup, Schematic capture and simulation
Lab 1: Cadence Custom IC design tools- Setup, Schematic capture and simulation Brittany Duffy EE 330- Integrated Electronics Lab Section B Professor Randy Geiger 1/24/13 Introduction The main goal of this
More informationEE115C Digital Electronic Circuits. Tutorial 4: Schematic-driven Layout (Virtuoso XL)
EE115C Digital Electronic Circuits Tutorial 4: Schematic-driven Layout (Virtuoso XL) This tutorial will demonstrate schematic-driven layout on the example of a 2-input NAND gate. Simple Layout (that won
More informationTUTORIAL II ECE 555 / 755 Updated on September 11 th 2006 CADENCE LAYOUT AND PARASITIC EXTRACTION
TUTORIAL II ECE 555 / 755 Updated on September 11 th 2006 CADENCE LAYOUT AND PARASITIC EXTRACTION After finishing a schematic of your design (Tutorial-I), the next step is creating masks which are for
More informationMentor Graphics VLSI CAD Tutorials
VLSI Design Flow Using Mentor-Graphics Tools Mentor Graphics VLSI CAD Tutorials School of Engineering Santa Clara University Santa Clara, CA 95053 At the Design Center, School of Engineering, of Santa
More informationFall 2008: EE5323 VLSI Design I using Cadence
1 of 23 9/17/2008 6:47 PM Fall 2008: EE5323 VLSI Design I using Cadence This tutorial has been adapted from EE5323 offered in Fall 2007. Thanks to Jie Gu, Prof. Chris Kim and Satish Sivaswamy of the University
More informationUsing Cadence Virtuoso, a UNIX based OrCAD PSpice like program, Remotely on a Windows Machine
Using Cadence Virtuoso, a UNIX based OrCAD PSpice like program, Remotely on a Windows Machine A. Launch PuTTY. 1. Load the Saved Session that has Enable X11 forwarding and the Host Name is cvl.ece.vt.edu.
More informationBasic Analog Simulation in Cadence
York University Department of Electrical Engineering and Computer Science EMIL Tutorial Series Tutorial #1 Basic Analog Simulation in Cadence In this tutorial we step through how to start Cadence (or at
More informationCadence IC Design Manual
Cadence IC Design Manual For EE5518 ZHENG Huan Qun Lin Long Yang Revised on May 2017 Department of Electrical & Computer Engineering National University of Singapore 1 P age Contents 1 INTRODUCTION...
More informationCadence Analog Circuit Tutorial
Cadence Analog Circuit Tutorial Schematic Entry for Analog Designs- Passive Circuits (RLC Circuit) In this tutorial, we will build the circuit shown in figure 1 below, using the Cadence Composer tool.
More informationVirtuoso Layout Editor
This tutorial will cover the basic steps involved in using the Cadence layout editor called Virtuoso, extracting layout, and running simulation on the layout. The inverter layout is used as an example
More informationFACULTY OF ENGINEERING MULTIMEDIA UNIVERSITY LAB SHEET DIGITAL INTEGRATED CIRCUIT
FACULTY OF ENGINEERING MULTIMEDIA UNIVERSITY LAB SHEET DIGITAL INTEGRATED CIRCUIT DIC1: Schematic Design Entry, Simulation & Verification DIC2: Schematic Driven Layout Drawing (SDL) Design Rule Check (DRC)
More informationELEC 301 Lab 2: Cadence Basic
ELEC 301 Lab 2: Cadence Basic Revision: 2.1 Last modified: Aug. 98 Introduction In this class, you will be introduced to the Cadence suit of IC design tools. These tools are a very powerful set of tools.
More informationVLSI Lab Tutorial 1. Cadence Virtuoso Schematic Composer Introduction
VLSI Lab Tutorial 1 Cadence Virtuoso Schematic Composer Introduction 1.0 Introduction The purpose of the first lab tutorial is to help you become familiar with the schematic editor, Virtuoso Schematic
More informationEE434 ASIC & Digital Systems. From Layout to SPICE Simulation (Virtuoso, Calibre, HSpice) Spring 2017 Dae Hyun Kim
EE434 ASIC & Digital Systems From Layout to SPICE Simulation (Virtuoso, Calibre, HSpice) Spring 2017 Dae Hyun Kim daehyun@eecs.wsu.edu 1 Preparation for Lab2 Download the following file into your working
More informationLogging in, starting a shell tool, and starting the Cadence Tool Suite
EEE 4134 VLSI I Laboratory Lab 0 (Introductory Lab) Logging into Cadence Server, Tool Setup, Cell Library Creation, Introduction to Custom IC Design flow Objectives: To login, start a shell tool and start
More informationEDA-BASED DESIGN PRACTICAL LABORATORY SESSION No. 3
LABORATOIRE DE SYSTEMES MICROELECTRONIQUES EPFL STI IMM LSM ELD Station nº 11 CH-1015 Lausanne Téléphone : Fax : E-mail : Site web : +4121 693 6955 +4121 693 6959 lsm@epfl.ch lsm.epfl.ch EDA-BASED DESIGN
More informationCadence Virtuoso Simulation of a pixel
MEMS AND MICROSENSORS 2018/2019 Cadence Virtuoso Simulation of a pixel 11/12/2018 Giorgio Mussi giorgio.mussi@polimi.it Introduction In this lab, we will use Cadence Virtuoso to simulate a sub-array of
More informationTUTORIAL 1. V1.1 Update on Sept 17, 2003 ECE 755. Part 1: Design Architect IC
TUTORIAL 1 V1.1 Update on Sept 17, 2003 ECE 755 Part 1: Design Architect IC DA-IC provides a design environment comprising tools to create schematics, symbols and run simulations. The schematic editor
More informationMicroelectronica. Full-Custom Design with Cadence Tutorial
Área Científica de Electrónica Microelectronica Full-Custom Design with Cadence Tutorial AustriaMicroSystems C35B3 (HIT-Kit 3.70) Marcelino Santos Table of contends 1. Starting Cadence... 3 Starting Cadence
More informationEE 140/240A - Full IC Design Flow Tutorial
Original document by Filip Maksimovic & Mike Lorek, Spring 2015, derived from earlier EE141 lab manuals Revisions for IC6 by David Burnett & Thaibao Phan, Spring 2016 Revisions made by Nandish Mehta to
More informationDC Circuit Simulation
Chapter 2 DC Circuit Simulation 2.1 Starting the Project Manager 1. Select Project Manager from the Start All Program Cadence Release 16.5 Project Manager. 2. Select Allegro PCB Designer (Schematic) from
More informationUniversity of Southern California EE 477L - MOS VLSI Circuit Design
University of Southern California EE 477L - MOS VLSI Circuit Design Contents 1. The Design Flow 2. Magic 3. IRSIM 4. HSPICE 5. Taking Printouts Brandon L Fernandes 2002 Design Flow in EE477L Step 1 Step
More informationExperiment 0: Introduction to Cadence
UNIVERSITY OF CALIFORNIA AT BERKELEY College of Engineering Department of Electrical Engineering and Computer Sciences EE105 Lab Experiments Experiment 0: Introduction to Cadence Contents 1. Introduction...
More informationEE5323/5324 VLSI Design I/II using Cadence
1 of 18 2009-1-23 23:58 Spring 2009: EE5323/5324 VLSI Design I/II using Cadence This tutorial has been adapted from EE5323 offered in Fall 2007. Thanks to Jie Gu, Prof. Chris Kim and Satish Sivaswamy of
More informationHow To Plot Transconductance and Even More. By Ruida Yun
How To Plot Transconductance and Even More By Ruida Yun g m /I d based methodology is preferred for short-channel length analog circuit design however there is no GUI support for this method in the current
More informationEE 105 Microelectronic Devices & Circuits FALL 2018 C. Nguyen
1. Objective UNIVERSITY OF CALIFORNIA College of Engineering Department of Electrical Engineering and Computer Sciences HSPICE Tutorial The objective of this session is to give initial exposure to the
More informationLab 5: Circuit Simulation with PSPICE
Page 1 of 11 Laboratory Goals Introduce text-based PSPICE as a design tool Create transistor circuits using PSPICE Simulate output response for the designed circuits Introduce the Tektronics 571 Curve
More informationHOMEWORK 9 CMPEN 411 Due: 4/12/ :30pm
HOMEWORK 9 CMPEN 411 Due: 4/12/2016 11:30pm Learning Objective Complete the full 8 bit RISC microprocessor chip design by placing the processor core design into the 40 pin 'tiny' chip pad frame. Do verify
More informationANALOG MICROELECTRONICS ( A)
ANALOG MICROELECTRONICS (304-534A) IBM 130 nm CMOS Technology An Introduction to Cadence Virtuoso Layout Tool and the Analog Simulation Environment Prepared By - Azhar A. Chowdhury Updated by Ming Yang
More informationGuide to the CSE 577 Lab and Cad tools
Guide to the CSE 577 Lab and Cad tools 1. Introduction The objective of this tutorial is to give you an overview to (1) setup the Cadence and Synopsys hspice tools for your account in IST 218 Lab, (2)
More informationEEC 116 Fall 2011 Lab #3: Digital Simulation Tutorial
EEC 116 Fall 2011 Lab #3: Digital Simulation Tutorial Dept. of Electrical and Computer Engineering University of California, Davis Issued: October 10, 2011 Due: October 19, 2011, 4PM Reading: Rabaey Insert
More informationIntroduction to CCV and Cadence Virtuoso for Electronic Circuit Simulation
Introduction to CCV and Cadence Virtuoso for Electronic Circuit Simulation Introduction ENGN1600 will be using the Cadence Virtuoso software suite for its circuit design and SPICE components. Part of the
More informationGetting started. Starting Capture. To start Capture. This chapter describes how to start OrCAD Capture.
Getting started 1 This chapter describes how to start OrCAD Capture. Starting Capture The OrCAD Release 9 installation process puts Capture in the \PROGRAM FILES\ORCAD\CAPTURE folder, and adds Pspice Student
More informationLab 4 LVS and Post layout Simulation
Lab 4 LVS and Post layout Simulation Objective: In this lab you will learn 1. How to check if your layout that you drew in lab 3 matches your schematic that you drew in lab 2. 2. How to do the post layout
More informationOPUS -- AMS 3.2. Version Manual
OPUS -- AMS 3.2 Version 4.4.3 Manual for students designing VLSI integrated circuits at the VLSI laboratory of the DED (V2-324) using the OPUS Design Environment on Sun workstations under the UNIX Operating
More informationRC Extraction. of an Inverter Circuit
RC Extraction of an Inverter Circuit Santa Clara University Department of Electrical Engineering Under Guidance of Dr Samiha Mourad & Dr Shoba Krishnan Date of Last Revision: February 1, 2010 Copyright
More informationCPE/EE 427, CPE 527, VLSI Design I: Tutorial #1, Full Custom VLSI (inverter layout)
CPE/EE 427, CPE 527, VLSI Design I: Tutorial #1, Full Custom VLSI (inverter layout) Joel Wilder, Aleksandar Milenkovic, ECE Dept., The University of Alabama in Huntsville Adapted from Virginia Tech, Dept.
More informationCPE/EE 427, CPE 527, VLSI Design I: Tutorial #4, Standard cell design flow (from verilog to layout, 8-bit accumulator)
CPE/EE 427, CPE 527, VLSI Design I: Tutorial #4, Standard cell design flow (from verilog to layout, 8-bit accumulator) Joel Wilder, Aleksandar Milenkovic, ECE Dept., The University of Alabama in Huntsville
More informationProcess technology and introduction to physical
Neuromorphic Engineering II Lab 3, Spring 2014 1 Lab 3 March 10, 2014 Process technology and introduction to physical layout Today you will start to learn to use the Virtuoso layout editor XL which is
More informationEE 330 Laboratory 3 Layout, DRC, and LVS Fall 2015
EE 330 Laboratory 3 Layout, DRC, and LVS Fall 2015 Contents Objective:... 2 Part 1 Creating a layout... 2 1.1 Run DRC Early and Often... 2 1.2 Create N active and connect the transistors... 3 1.3 Vias...
More informationHOMEWORK 10 CMPEN 411 Due: 4/28/ :30pm
HOMEWORK 10 CMPEN 411 Due: 4/28/2016 11:30pm Instruction First, fabrication ready the full 8 bit RISC microprocessor chip: redesign the chip (its components) to fit the entire chip fitted into the 40 pin
More informationMENTOR GRAPHICS IC DESIGN MANUAL. Schematic & Simulation. Gun Jun K Praveen Jayakar Thomas Zheng Huan Qun
MENTOR GRAPHICS IC DESIGN MANUAL Schematic & Simulation By Gun Jun K Praveen Jayakar Thomas Zheng Huan Qun August 2004 Signal Processing & VLSI Design Laboratory Department of Electrical & Computer Engineering
More informationAPPENDIX-A INTRODUCTION TO OrCAD PSPICE
220 APPENDIX-A INTRODUCTION TO OrCAD PSPICE 221 APPENDIX-A INTRODUCTION TO OrCAD PSPICE 1.0 INTRODUCTION Computer aided circuit analysis provides additional information about the circuit performance that
More informationPSpice Tutorial. Physics 160 Spring 2006
PSpice Tutorial This is a tutorial designed to guide you through the simulation assignment included in the first homework set. You may either use the program as installed in the lab, or you may install
More informationVLSI Lab Tutorial 3. Virtuoso Layout Editing Introduction
VLSI Lab Tutorial 3 Virtuoso Layout Editing Introduction 1.0 Introduction The purpose of this lab tutorial is to guide you through the design process in creating a custom IC layout for your CMOS inverter
More informationDesign rule illustrations for the AMI C5N process can be found at:
Cadence Tutorial B: Layout, DRC, Extraction, and LVS Created for the MSU VLSI program by Professor A. Mason and the AMSaC lab group. Revised by C Young & Waqar A Qureshi -FS08 Document Contents Introduction
More informationLaboratory 6. - Using Encounter for Automatic Place and Route. By Mulong Li, 2013
CME 342 (VLSI Circuit Design) Laboratory 6 - Using Encounter for Automatic Place and Route By Mulong Li, 2013 Reference: Digital VLSI Chip Design with Cadence and Synopsys CAD Tools, Erik Brunvand Background
More informationCadence Inverter Transistor Sizing Tutorial Cadence Inverter Ocean Introduction Cadence Inverter Corners Tutorial Cadence Inverter VerilogA Tutorial
Cadence Inverter Transistor Sizing Tutorial Cadence Inverter Ocean Introduction Cadence Inverter Corners Tutorial Cadence Inverter VerilogA Tutorial Alfred Sargezi & Zain Ali AMS Group - San Jose State
More informationThis is a brief tutorial about building a Symbol for a Schematic in Cadence IC design tool environment for hierarchical design of schematics.
This is a brief tutorial about building a Symbol for a Schematic in Cadence IC design tool environment for hierarchical design of schematics. 1. > cd work035 2. > cadsetup ams035 3. > virtuoso& IMPORTANT:
More informationDRC and LVS checks using Cadence Virtuoso Version 2.0
DRC and LVS checks using Cadence Virtuoso Version 2.0 Start virtuoso l l Open a virtuoso session in the directory which contains the required cds.lib and lib.def files. Command : virtuoso & Open the layout
More information