Random Vibration Analysis of a Circuit Board. Sean Harvey August 2000 CSI Tip of the Week
|
|
|
- Arlene Harris
- 5 years ago
- Views:
Transcription
1 Random Vibration Analysis of a Circuit Board Sean Harvey August 2000 CSI Tip of the Week
2 Random Vibrations Outline Introduction Sample Problem Description Pre Processing Steps Omitted Interactive steps Specify Modal Analysis Specify Modal Analysis Options Constrain Board Solve Modal Specify Spectrum Analysis Specify Analysis Options Specify PSD Settings Specify PSD vs. Frequency (Continued) Plot Input PSD Specify Damping Flag Nodes to get PSD Input Solve for Participation Factors Set PSD Calculation Controls Solve Random Vibration Solution Set Mode Combination Calculate mode combinations and 1 sigma response Post Processing Results Summary 1 sigma Results Post Processing 1 sigma Displacements Post Processing 1 sigma Stresses Plotting Response PSD in Post 26
3 Introduction What is a Random Vibration Analysis? A Random Vibration Analysis is a form of Spectrum Analysis. The spectrum is a graph of spectral value versus frequency that captures the intensity and frequency content of time-history loads. Random vibration analysis is probabilistic in nature, because both input and output quantities represent only the probability that they take on certain values.
4 Introduction What is a Random Vibration Analysis (continued)? Random Vibration Analysis uses Power spectral density to quantify the loading. (PSD) is a statistical measure defined as the limiting mean-square value of a random variable. It is used in random vibration analyses in which the instantaneous magnitudes of the response can be specified only by probability distribution functions that show the probability of the magnitude taking a particular value.
5 Introduction What is a PSD Spectrum? A PSD spectrum is a statistical measure of the response of a structure to random dynamic loading conditions. It is a graph of the PSD value versus frequency, where the PSD may be a displacement PSD, velocity PSD, acceleration PSD, or force PSD. Mathematically, the area under a PSD-versus-frequency curve is equal to the variance (square of the standard deviation of the response).
6 Introduction Sample PSD Curves Sample Acceleration PSD Curve Sample Acceleration PSD Curve PSD (g^2/hz) PSD (g^2/hz) Frequency (Hz) Frequency (Hz)
7 Introduction How does one obtain a PSD Spectrum? PSD spectrum curves are generally supplied as a spec., or are measured and calculated using vibration analysis equipment.
8 Sample Problem The following steps will detail running through a simple PSD analysis using the GUI. An input file with every command is included at the end of this document...
9 Sample Problem Description Circuit Board exposed to a Base Acceleration Power Spectral Density (g^2/hz) input in the global Z direction (normal to board) on 4 corners as show below; Input Acceleration PSD 0.06 PSD PSD PSD (g^2/hz) PSD 0.01 PSD Frequency (Hz)
10 Sample Problem Description Circuit Board with 3 components Board Constrained at 4 corners in all DOF Damping Ratio = 2% Model meshed with Solid92 10 noded tetrahedrons
11 Sample Problem Description Preprocessing steps - Details omitted Import Geometry, Glue Volumes, Define Material Properties, Assign Material Attributes, Set Element Type, Mesh Model. Solution steps - Step by Step starting on next slide...
12 Specify Modal Analysis ANSYS Main Menu> Solution > New Analysis Pick Modal
13 Specify Modal Analysis Options ANSYS Main Menu> Solution > Analysis Options Pick Modal Extraction Method (Block Lanczos a good choice) Specify 20 modes to extract Expand all modes Calculate Element results
14 Constrain Board ANSYS Main Menu> Solution > Apply > Displacement > On Nodes Pick the 4 corner nodes on the bottom side of the board Constrain All DOF (UX,UY,UZ)
15 Solve Modal ANSYS Main Menu> Solution > Solve
16 Specify Spectrum Analysis ANSYS Main Menu> Finish ANSYS Main Menu> Solution > New Analysis Pick Spectrum
17 Specify Analysis Options ANSYS Main Menu> Solution > Analysis Options Specify P.S.D Specify the number of modes from the modal to include in the PSD analysis. Specify to Calculate Element Results (stresses, strains,etc.)
18 Specify PSD Settings ANSYS Main Menu> Solution > Spectrum > PSD > Settings Input data will be in terms of g^2/hz, therefore specify this setting Analysis has one PSD table, therefore leave table number to 1 Specify Value of acceleration due to gravity (g)
19 Specify PSD vs. Frequency ANSYS Main Menu> Solution > Spectrum > PSD > PSD vs. Freq Specify 1 for the PSD Table (only one table in this analysis) Enter Frequency and Value data
20 Plot Input PSD ANSYS Main Menu> Solution > Spectrum > PSD > Plot Set table to 1
21 Specify Damping ANSYS Main Menu> Solution > Time/Frequency > Damping Specify 2% Constant Damping Ratio
22 Flag Nodes to get PSD Input ANSYS Main Menu> Solution > Apply > Spectrum > Base PSD Excit > On Nodes Pick the 4 corner nodes on the bottom side of the board
23 Flag Nodes to get PSD Input ANSYS Main Menu> Solution > Apply > Spectrum > Base PSD Excit > On Nodes Specify Excitation direction to Z Note: This will flag a 1 displacement on the node telling ANSYS the previously defined PSD table is to be applied. You can apply base excitations only at nodes that were constrained in the modal analysis. UX,UY =0 Constraints on these 4 nodes are left over from Modal Analysis, and remain through PSD Analysis. No need to respecify them.
24 Solve for Participation Factors ANSYS Main Menu> Solution > Apply > Spectrum > Calculate PF... Specify 1 for table Specify Base excitation Problem Leave parcor to default. Not required for single PSD excitation Note: This step Calculates the participation factors for the specified PSD table
25 Set PSD Calculation Controls ANSYS Main Menu> Solution > Spectrum > PSD > Calc Controls Specify all Solution items are to be calculated Relative to Base. This means the input excitation is subtracted out. Input nodes have their results reported as zero. Note: These specifications are for the general postprocessor results, not the time history postprocessor.
26 Solve Random Vibration Solution ANSYS Main Menu> Solution > Solve > Current LS
27 ANSYS Main Menu> Finish Set Mode Combination ANSYS Main Menu> Solution > Spectrum > PSD > Mode Combine... Leave significance at 0. All 20 modes will be used in mode combination
28 Calculate mode combinations and 1 sigma response ANSYS Main Menu> Solution > Solve > Current LS
29 Post Processing Results Summary ANSYS Main Menu> General Post Processor > Results Summary Load step 1 - modal results Load step 2 - unit static solutions Load step 3-1 sigma displacements, strains, stresses Load step 4-1 sigma velocities Load step 5-1 sigma accelerations
30 1 sigma Results 1σ results are typically used for: First passage failure calculations What is the probability that the displacement at a DOF will exceed a displacement limit in a given time period? Fatigue calculations Based on the premise that the stress level is at or below 1σ 68.2% of the time, between 1σ=and 2σ 27.2% of the time ( ), and between 2σ=and 3σ 4.3% of the time ( ), and above 3σ=less than.3% of the time.
31 Post Processing 1 sigma Displacements ANSYS Main Menu> General Post Processor > Plot Results > Nodal Solution >DOF Solution > USUM 1 sigma board deflection = sigma board deflection = 3 *.002 =.006 Therefore, only.3% of the time, board deflection will exceed.006
32 Post Processing 1 sigma Stresses ANSYS Main Menu> General Post Processor > Plot Results > Nodal Solution >Stress > SEQV 1 sigma corner stress = 698 psi 3 sigma corner stress = 3 *. 698 psi= 2094 psi Therefore, only.3% of the time, board corner stress will exceed 2094 psi Note: For simplicity in this model, the corner nodes are constrained. This creates singular stress results. In reality, modeling and holding the actual mounting hold would provide more accurate results.
33 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Store Data This command sets the resolution of the frequency vector for the PSD curve. 10 gives finer results 1 gives coarser results. 5 is the default.
34 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Define Variables This command defines the variables that we want to see as a function of time or frequency
35 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Define Variables Pick one corner node that was constrained is picked in this case.
36 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Define Variables Specify UZ DOF and specify a label, in this case label is called base.
37 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Define Variables Pick node 350 on top of component
38 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Define Variables Specify UZ DOF and specify a label, in this case label is called Node_350.
39 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Calculate Resp PSD Specify new variable number to store PSD in Specify existing variable number that has DOF solution. In this case 2 is the corner node base excitation. Specify the response to be acceleration. Specify absolute in order to plot input PSD and response PSD together Give new variable a label
40 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Calculate Resp PSD Specify new variable number to store PSD in Specify existing variable number that has DOF solution. In this case 3 is the node on top of a component Specify the response to be acceleration. Specify absolute in order to plot input PSD and response PSD together Give new variable a label
41 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Math Operations Convert results from in^2/sec^4/hz into g^2/hz by dividing results by 1/g^2 = 1/386.4**2 Specify variable 7 gets the results of this operation Specify 1/g^2 factor Specify variable 4 to operate on. This has the input PSD in in^2/sec^4/hz Give new variable a label
42 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Math Operations Convert results from in^2/sec^4/hz into g^2/hz by dividing results by 1/g^2 = 1/386.4**2 Specify variable 8 gets the results of this operation Specify 1/g^2 factor Specify variable 5 to operate on. This has the component node PSD in in^2/sec^4/hz Give new variable a label
43 Plotting Response PSD in Post 26 Plot Controls > Style > Graphs > Modify Axes Define labels for graph Set axes to Logarithmic
44 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Graph Variables Plot input PSD (g^2/hz) variable 7 Plot response PSD (g^2/hz) variable 8
45 Plotting Response PSD in Post 26 ANSYS Main Menu> Time History Post Processor > Graph Variables Plot shows the response PSD of the component on the board versus the input PSD at one of the corner nodes. From this plot we see the dynamic amplification the circuit board provides from the input PSD.
Figure Random vibration analysis of a simply supported beam
Example 6.5.8-1 [Spectrum Analysis] Determine the first two natural frequencies and the response of a damped two degree of freedom system subject to a random acceleration with a spectral density function
CHAPTER 5 RANDOM VIBRATION TESTS ON DIP-PCB ASSEMBLY
117 CHAPTER 5 RANDOM VIBRATION TESTS ON DIP-PCB ASSEMBLY 5.1 INTRODUCTION Random vibration tests are usually specified as acceptance, screening and qualification tests by commercial, industrial, and military
Institute of Mechatronics and Information Systems
EXERCISE 4 Free vibrations of an electrical machine model Target Getting familiar with the fundamental issues of free vibrations analysis of a simplified model of an electrical machine, with the use of
Structural modal analysis - 2D frame
Structural modal analysis - 2D frame Determine the first six vibration characteristics, namely natural frequencies and mode shapes, of a structure depicted in Fig. 1, when Young s modulus= 27e9Pa, Poisson
Two Dimensional Truss
Two Dimensional Truss Introduction This tutorial was created using ANSYS 7.0 to solve a simple 2D Truss problem. This is the first of four introductory ANSYS tutorials. Problem Description Determine the
NonLinear Materials AH-ALBERTA Web:
NonLinear Materials Introduction This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model. For instance, the case
Institute of Mechatronics and Information Systems
EXERCISE 2 Free vibrations of a beam arget Getting familiar with the fundamental issues of free vibrations analysis of elastic medium, with the use of a finite element computation system ANSYS. Program
Rigid Dynamic Analysis in Workbench
Rigid Dynamic Analysis in Workbench 1-1 Introduction Rigid Dynamic Analysis: Calculates dynamic response of an assembly of rigid bodies. Can be used to study the kinematics of an assembly. Bodies are linked
Tutorial for Response Spectrum Analysis using CAEPIPE
Tutorial for Response Spectrum Analysis using CAEPIPE The following are the Steps for performing the Response Spectrum Analysis using CAEPIPE. General The Response Spectrum is a plot of the maximum response
Structural static analysis - Analyzing 2D frame
Structural static analysis - Analyzing 2D frame In this tutorial we will analyze 2D frame (see Fig.1) consisting of 2D beams with respect to resistance to two different kinds of loads: (a) the downward
A pipe bend is subjected to a concentrated force as shown: y All dimensions in inches. Material is stainless steel.
Problem description A pipe bend is subjected to a concentrated force as shown: y 15 12 P 9 Displacement gauge Cross-section: 0.432 18 x 6.625 All dimensions in inches. Material is stainless steel. E =
Exercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method
Exercise 1 3-Point Bending Using the GUI and the Bottom-up-Method Contents Learn how to... 1 Given... 2 Questions... 2 Taking advantage of symmetries... 2 A. Preprocessor (Setting up the Model)... 3 A.1
ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis
R50 ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis Example 1 Static Analysis of a Bracket 1. Problem Description: The objective of the problem is to demonstrate the basic ANSYS procedures
Bracket (Modal Anslysis)
(Modal Anslysis) Chapter Overview The sample session described in this chapter demonstrates a simple linear static and dynamic analysis on a steel bracket. The bracket restrains a vertical pipe. The bracket
Generative Part Structural Analysis Expert
CATIA V5 Training Foils Generative Part Structural Analysis Expert Version 5 Release 19 September 2008 EDU_CAT_EN_GPE_FI_V5R19 About this course Objectives of the course Upon completion of this course
Parametric. Practices. Patrick Cunningham. CAE Associates Inc. and ANSYS Inc. Proprietary 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved.
Parametric Modeling Best Practices Patrick Cunningham July, 2012 CAE Associates Inc. and ANSYS Inc. Proprietary 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. E-Learning Webinar Series This
Structural modal analysis - 2D frame
Structural modal analysis - 2D frame Determine the first six vibration characteristics, namely natural frequencies and mode shapes, of a structure depicted in Fig. 1, when Young s modulus= 27e9Pa, Poisson
Finite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench
Finite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench Course Curriculum (Duration: 120 Hrs.) Section I: ANSYS Mechanical APDL Chapter 1: Before you start using ANSYS a. Introduction to
ECE421: Electronics for Instrumentation
ECE421: Electronics for Instrumentation Lecture #8: Introduction to FEA & ANSYS Mostafa Soliman, Ph.D. March 23 rd 2015 Mostafa Soliman, Ph.D. 1 Outline Introduction to Finite Element Analysis Introduction
PTC Newsletter January 14th, 2002
PTC Email Newsletter January 14th, 2002 PTC Product Focus: Pro/MECHANICA (Structure) Tip of the Week: Creating and using Rigid Connections Upcoming Events and Training Class Schedules PTC Product Focus:
Chapter 2. Structural Tutorial
Chapter 2. Structural Tutorial Tutorials> Chapter 2. Structural Tutorial Static Analysis of a Corner Bracket Problem Specification Problem Description Build Geometry Define Materials Generate Mesh Apply
Module 1.6: Distributed Loading of a 2D Cantilever Beam
Module 1.6: Distributed Loading of a 2D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing
file://c:\documents and Settings\sala\Configuración local\temp\~hha54f.htm
Página 1 de 26 Tutorials Chapter 2. Structural Tutorial 2.1. Static Analysis of a Corner Bracket 2.1.1. Problem Specification Applicable ANSYS Products: Level of Difficulty: Interactive Time Required:
NX Response Simulation: Structural dynamic response
Response Simulation: Structural dynamic response NX CAE Benefits Reduce costly physical prototypes by using response simulation to improve product performance Gain insight into the dynamic response of
Module 1.5: Moment Loading of a 2D Cantilever Beam
Module 1.5: Moment Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Loads
Module 1.2: Moment of a 1D Cantilever Beam
Module 1.: Moment of a 1D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry Preprocessor 6 Element Type 6 Real Constants and Material Properties 7 Meshing 9 Loads 10 Solution
Contents. 1 Introduction. 2 Theoretical Background
Contents 1 Introduction Introduction........................................ 1-1 Analysis Capabilities................................. 1-2 Main Analysis Features............................... 1-2 Load
Structural static analysis - Analyzing 2D frame
Structural static analysis - Analyzing 2D frame In this tutorial we will analyze 2D frame (see Fig.1) consisting of 2D beams with respect to resistance to two different kinds of loads: (a) the downward
ANSYS Workbench Guide
ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through
NonLinear Analysis of a Cantilever Beam
NonLinear Analysis of a Cantilever Beam Introduction This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to do a simple nonlinear analysis of the beam
Retrieve Beam Reaction Forces In ANSYS Random Vibration Analysis
Retrieve Beam Reaction Forces In ANSYS Random Vibration Analysis ANSYS Workbench (WB) Mechanical provides the ability to perform random vibration analyses, which are sometimes referred to as power spectral
FEM Modeling: Mesh, Loads
8 FEM Modeling: Mesh, Loads and BCs IFEM Ch 8 Slide 1 Topics in Chapter 8 General Modeling Rules Finite Element Mesh Layouts Distributed Loads Displacement BCs suppressing rigid body motions taking advantage
Transient Thermal Conduction Example
Transient Thermal Conduction Example Introduction This tutorial was created using ANSYS 7.0 to solve a simple transient conduction problem. Special thanks to Jesse Arnold for the analytical solution shown
Module 1.7: Point Loading of a 3D Cantilever Beam
Module 1.7: Point Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 6 Element Type 6 Material Properties 7 Meshing 8 Loads 9 Solution 15 General
The Vibration Characteristics Analysis of Damping System of Wallmounted Airborne Equipment Based on FEM
IOP Conference Series: Earth and Environmental Science PAPER OPEN ACCESS The Vibration Characteristics Analysis of Damping System of Wallmounted Airborne Equipment Based on FEM To cite this article: Changqing
Case Study 2: Piezoelectric Circular Plate
Case Study 2: Piezoelectric Circular Plate PROBLEM - 3D Circular Plate, kp Mode, PZT4, D=50mm x h=1mm GOAL Evaluate the operation of a piezoelectric circular plate having electrodes in the top and bottom
Course in ANSYS. Example0410. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0410 Example Frame 2D Objective: Compute the harmonic response Tasks: Perform a modal analysis Display the mode shapes Perform a harmonic analysis Topics: Topics: Start of analysis, Element
Example Cantilever beam
Course in ANSYS Example0300 Example Cantilever beam Objective: Compute the maximum deflection and locate point of maximum deflection Tasks: How should this be modelled? Compare results with results obtained
TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS.
Ex_1_2D Plate.doc 1 TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. 1. INTRODUCTION Two-dimensional problem of the theory of elasticity is a particular
MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1
Instructions MAE 323 Lab Instructions 1 Problem Definition Determine how different element types perform for modeling a cylindrical pressure vessel over a wide range of r/t ratios, and how the hoop stress
Engineering Analysis
Engineering Analysis with SOLIDWORKS Simulation 2018 Paul M. Kurowski SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites
Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA
Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA Andrew Smyth, P.E. LPI, Inc., New York, NY, USA Abstract Overhead crane wire ropes utilized within manufacturing plants are subject to extensive
Analysis of Pile Behaviour due to Damped Vibration by Finite Element Method (FEM)
ISSN 2395-1621 Analysis of Pile Behaviour due to Damped Vibration by Finite Element Method (FEM) #1 L.M.Sardesai, #2 G.A.Kadam 1 sardesaileena@rediffmail.com.com 2 ganeshkadam07@gmail.com #1 Mechanical
ANSYS Mechanical Basic Structural Nonlinearities
Workshop 4A Metal Plasticity 14. 0 Release ANSYS Mechanical Basic Structural Nonlinearities 1 Goal: Workshop 4A Metal Plasticity Define a nonlinear metal plasticity material for a belleville spring geometry
Defining the Global Error of a Multi-Axis Vibration Test: An Application of MIL-STD-810G Method 527 Annex C
Defining the Global Error of a Multi-Axis Vibration Test: An Application of MIL-STD-810G Method 527 Annex C Joel Hoksbergen Team Corporation joel.hoksbergen@teamcorporation.com ESTECH 2014 MIMO Concepts
CHAPTER 8 FINITE ELEMENT ANALYSIS
If you have any questions about this tutorial, feel free to contact Wenjin Tao (w.tao@mst.edu). CHAPTER 8 FINITE ELEMENT ANALYSIS Finite Element Analysis (FEA) is a practical application of the Finite
Modal Transient Response Analysis
WORKSHOP PROBLEM 4 Modal Transient Response Analysis Z Y X Objectives Create a geometric representation of a flat rectangular plate. Use the geometry model to define an analysis model comprised of plate
COMPUTER AIDED ENGINEERING. Part-1
COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.
Chapter 3. Thermal Tutorial
Chapter 3. Thermal Tutorial Tutorials> Chapter 3. Thermal Tutorial Solidification of a Casting Problem Specification Problem Description Prepare for a Thermal Analysis Input Geometry Define Materials Generate
6. Results Combination in Hexagonal Shell
6. Results Combination in Hexagonal Shell Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 0 minutes Discipline: Load combinations results Analysis
Femap Version
Femap Version 11.3 Benefits Easier model viewing and handling Faster connection definition and setup Faster and easier mesh refinement process More accurate meshes with minimal triangle element creation
VALIDATION OF SASSI2010 SOLUTION METHODS THROUGH INDEPENDENT VERIFICATION USING SAP2000 FOR DEEPLY EMBEDDED STRUCTURES WITH LARGE FOOTPRINTS
Transactions, SMiRT-22 VALIDATION OF SASSI2010 SOLUTION METHODS THROUGH INDEPENDENT VERIFICATION USING SAP2000 FOR DEEPLY EMBEDDED STRUCTURES WITH LARGE FOOTPRINTS Lisa M Anderson 1, Tarek Elkhoraibi,
ANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved.
ANSYS Element Selection elearning Peter Barrett October 2012 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection What is the best element type(s) for my analysis? Best
Course in ANSYS. Example0303. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0303 Example Gear axle 3D Objective: Compute the maximum stress von Mise Tasks: How should this be modeled? Topics: Element type, Real constants, modeling, Plot results, output graphics,
Webinar: Sesam and Bladed - Efficient coupled analyses
QUESTIONS AND ANSWERS Webinar: Sesam and Bladed - Efficient coupled analyses PRESENTERS: Laurens Alblas, Technical Support Engineer and William Collier, Senior Engineer DATE: 28 September 2017 1. Is this
Coustyx Tutorial Indirect Model
Coustyx Tutorial Indirect Model 1 Introduction This tutorial is created to outline the steps required to compute radiated noise from a gearbox housing using Coustyx software. Detailed steps are given on
Rotordynamics in ANSYS
Rotordynamics in ANSYS 1 ASME Turbo Expo 2013 Dave Looman Tech. Support Mgr. Rotordynamics in ANSYS - Outline Introduction ANSYS Rotordynamics capabilities by analysis type Continuing Rotordynamics Enhancements
300 N All lengths in meters. Step load applied at time 0.0.
Problem description In this problem, we subject the beam structure of problem 1 to an impact load as shown. 300 N 0.02 0.02 1 All lengths in meters. Step load applied at time 0.0. E = 2.07 10 11 N/m 2
Example Plate with a hole
Course in ANSYS Example Plate with a hole A Objective: Determine the maximum stress in the x-direction for point A and display the deformation figure Tasks: Create a submodel to increase the accuracy of
The ECHO commands. Synopsis. Syntax
The ECHO commands Synopsis The ECHO commands are used to control the verification or echo printing of various portions of the input data The ECHO commands have no effect on the results of an analysis Syntax
SMSIM Calibration for the SCEC Validation Project NGA-East Workshop Berkeley 12/11/12
SMSIM Calibration for the SCEC Validation Project NGA-East Workshop Berkeley 12/11/12 SWUS GMC SSHAC Level 3 Carola Di Alessandro GeoPentech with inputs from D.M. Boore OUTLINE Introduce SMSIM (Stochastic
Getting Started. These tasks should take about 20 minutes to complete. Getting Started
Getting Started Getting Started This tutorial will guide you step-by-step through your first ELFINI and Generative Part Structural Analysis session, allowing you to get acquainted with the product. You
KINETICS Vibration Isolation Manual
The Pitfalls of Combining Internal & External Equipment Isolation Introduction: Almost all Make-up Air Units (MAU), Air Handling Units (AHU), and Rooftop Units (RTU) have internal spring-type isolation
Nonlinear Convergence
Twin Cities ANSYS User Meeting November 2010 Nonlinear Convergence Content by Epsilon FEA, LLC Nonlinear Convergence Types of Nonlinearities 1. High Deformation (NLGEOM) 2. Contact 3. Material Types of
Problem description C L. Tank walls. Water in tank
Problem description A cylindrical water tank is subjected to gravity loading and ground accelerations, as shown in the figures below: Tank walls Water in tank Wall thickness 0.05 C L 5 g=9.81 m/s 2 Water:
About the Author. Acknowledgements
About the Author Dr. Paul Kurowski obtained his MSc and PhD in Applied Mechanics from Warsaw Technical University. He completed postdoctoral work at Kyoto University. Dr. Kurowski is an Assistant Professor
DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION
DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION 7 DYNAMIC ANALYSIS OF A GENERATOR ON AN ELASTIC FOUNDATION In this tutorial the influence of a vibrating source on its surrounding soil is studied.
CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the
Course in ANSYS. Example0153. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0153 Example Offshore structure F Objective: Display the deflection figure and von Mises stress distribution Tasks: Import geometry from IGES. Display the deflection figure? Display the
Design Analysis Of Industrial Gear Box Casing.
Design Analysis Of Industrial Gear Box Casing. Balasaheb Sahebrao Vikhe 1 1 Assistant Professor, Dept. of Mechanical Engineering, SVIT College Nasik, Maharashtra, India ---------------------------------------------------------------------***---------------------------------------------------------------------
WinFElt Manual. Problem description
WinFElt Manual Problem description The problem description section is used to define the problem title and the number of nodes and elements in the problem. The problem description section is the only section
A Simplified Vehicle and Driver Model for Vehicle Systems Development
A Simplified Vehicle and Driver Model for Vehicle Systems Development Martin Bayliss Cranfield University School of Engineering Bedfordshire MK43 0AL UK Abstract For the purposes of vehicle systems controller
Ansys Mechanical APDL
Ansys Mechanical APDL Day 1: FEA and ANSYS 9.00 12.00 About ANSYS, What is FEA?, Instructor Example Getting Started 12.00 1.00 Interactive Vs. Batch Mode, Starting ANSYS, Product Launcher, ANSYS Workbench,
Module 3: Buckling of 1D Simply Supported Beam
Module : Buckling of 1D Simply Supported Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Solution
Best Practices for Contact Modeling using ANSYS
Best Practices for Contact Modeling using ANSYS 朱永谊 / R&D Fellow ANSYS 1 2016 ANSYS, Inc. August 12, 2016 ANSYS UGM 2016 Why are these best practices important? Contact is the most common source of nonlinearity
3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation
3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack
m+p VibControl Random Vibration Control
www.mpihome.com m+p VibControl Random Vibration Control m+p VibControl is m+p international s proven software for carrying out a wide variety of vibration tests. The Random control mode is one of the most
ANSYS Tutorial Version 6
ANSYS Tutorial Version 6 Fracture Analysis Consultants, Inc www.fracanalysis.com Revised: November 2011 Table of Contents: 1.0 Introduction... 4 2.0 Tutorial 1: Crack Insertion and Growth in a Cube...
Introduction to the Finite Element Method (3)
Introduction to the Finite Element Method (3) Petr Kabele Czech Technical University in Prague Faculty of Civil Engineering Czech Republic petr.kabele@fsv.cvut.cz people.fsv.cvut.cz/~pkabele 1 Outline
FEA Applications I MET 415 Review Course Structure: 15 week course Weekly Schedule 50 minute lecture 2.5 hour laboratory 50 minute lecture
FEA Applications I MET 415 Review Course Structure: 15 week course Weekly Schedule 50 minute lecture 2.5 hour laboratory 50 minute lecture Goal: Obtain feedback from Industry Users on course presentation
Element Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can
TIPS www.ansys.belcan.com 鲁班人 (http://www.lubanren.com/weblog/) Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be
ME Week 12 Piston Mechanical Event Simulation
Introduction to Mechanical Event Simulation The purpose of this introduction to Mechanical Event Simulation (MES) project is to explorer the dynamic simulation environment of Autodesk Simulation. This
Krzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004
Structural stability of shelf probe cards Krzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004 Presentation Outline Introduction Objectives Multi die applications
Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses
Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses Goals In this exercise, we will explore the strengths and weaknesses of different element types (tetrahedrons vs. hexahedrons,
11. Push-over analysis
. Push-over analysis Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 90 minutes Discipline: Structural Steel Analysis Type: Push Over Element
Using Impulse Response Functions to Evaluate Baseball Bats
Using Impulse Response Functions to Evaluate aseball ats David L. Formenti David Ottman Mark H. Richardson lackhawk Technology, Inc. Hillerich & radsby o. Vibrant Technology, Inc Santa ruz, A Loomis, A
Materials, Load Cases and LBC Assignment
LESSON 4 Materials, Load Cases and LBC Assignment 5.013 5.000 4.714 30000 4.429 4.143 3.858 3.572 3.287 3.001 2.716 2.430 2.145 1.859 20000 1.574 1.288 default_fringe : 1.003 Max 2.277 @Elm 40079.1 Min
Hourglass (HG) Modes. Hourglass (HG) Modes
Hourglass (HG) Modes Hourglass modes are nonphysical modes of deformation that occur in underintegrated elements and produce no stress. By underintegrated, we mean Solid elements with a single integration
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
ANSYS 6.0 Variable Viewer
ANSYS 6.0 Variable Viewer New Variable Viewer to Review Time-History Data New Time-History Commands New XY-Plotting Graphing Options Overview of 6.0 Enhancements A number of enhancements for time-history
Generative Part Structural Analysis Fundamentals
CATIA V5 Training Foils Generative Part Structural Analysis Fundamentals Version 5 Release 19 September 2008 EDU_CAT_EN_GPF_FI_V5R19 About this course Objectives of the course Upon completion of this course
WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14
WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.
SIMULATION CAPABILITIES IN CREO
SIMULATION CAPABILITIES IN CREO Enhance Your Product Design with Simulation & Using digital prototypes to understand how your designs perform in real-world conditions is vital to your product development
Optimization to Reduce Automobile Cabin Noise
EngOpt 2008 - International Conference on Engineering Optimization Rio de Janeiro, Brazil, 01-05 June 2008. Optimization to Reduce Automobile Cabin Noise Harold Thomas, Dilip Mandal, and Narayanan Pagaldipti
ANSYS Tutorials. Table of Contents. Grady Lemoine
ANSYS Tutorials Grady Lemoine Table of Contents Example 1: 2-D Static Stress Analysis in ANSYS...2 Example 2: 3-D Static Stress Analysis...5 Example 3: 2-D Frame With Multiple Materials and Element Types...10
From Motion diagrams to Position and Velocity Graphs
From Motion diagrams to Position and Velocity Graphs Name: Group Members: Date: TA s Name: Apparatus: Aluminum track and a support, cart, plastic ruler, tape timer, and pencil Objectives: 1) To be familiar
Modal Analysis of Exhaust System to Optimize Mounting Hanger Location
Modal Analysis of Exhaust System to Optimize Mounting Hanger Location Chetan D. Gaonkar Assistant Professor, Mechanical Engineering Dpt., DBCE, Margao, Goa Abstract An exhaust system with a superior performance
Odysseas Skartsis ENGN2340. Project LEFM Convergence Study 12/11/13
Odysseas Skartsis ENGN2340 Project LEFM Convergence Study 2//3 Thanks to Tianyang Zhang, Davide Grazioli, and Ruike Zhao for their helpful tips on using ABAQUS. Structure of this report Main body: Appendix:
How to Achieve Quick and Accurate FE Solution Small Radius Removal and Element Size
How to Achieve Quick and Accurate FE Solution Small Radius Removal and Element Size Zhichao Wang - Sr. Lead Engineer Don Draper - Manager Jianxiong Chen Sr. Engineering Specialist Applied Mechanics Dept.,
5. Shell Reinforcement According To Eurocode 2
5. Shell Reinforcement According To Eurocode Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 5 minutes Discipline: Concrete Shell Reinforcement