ME 475 FEA of a Composite Panel

Size: px
Start display at page:

Download "ME 475 FEA of a Composite Panel"

Transcription

1 ME 475 FEA of a Composite Panel Objectives: To determine the deflection and stress state of a composite panel subjected to asymmetric loading. Introduction: Composite laminates are composed of thin layers (plies) consisting of reinforcement and a matrix. The reinforcement are typically a strong, stiff material, in the form of long fibers. The matrix is typically a material that is applied in a liquid form and then cured and hardened. The matrix is applied to support the reinforcement, and to distribute the load through the reinforcement and plies. It is common to have plies with fibers in one direction, also called unidirectional, or in several directions in a weave. The orientation of the fibers and stacking sequence has a large effect on the deformation and stress throughout the laminate. The stress in a laminate is more complex to characterize than that for linearly elastic, homogeneous, isotropic (LEHI) materials. It is discontinuous through the plies, and thus must be evaluated differently. Failure, consequently, is also much more complex than for LEHI materials, and will not be discussed in this class. In this lab, a foam core between two laminates will be utilized. This is a common practice, since it puts the fibers farther from the center of the plate. This increases the bending stiffness of the laminate, while only adding a small amount of mass (ρ foam << ρ laminate ). Analysis Problem Statement: A composite panel made of four plies of carbon/epoxy above and below a foam core. The panel is cantilevered, and has a point load applied to one corner, as shown in Figure 1. 1

2 10000 N Carbon/epoxy unidirectional laminate: E 1 = 147 GPa, E 2 = E 3 = 10.3 GPa ν 12 = ν 13 = 0.27, ν 23 = 0.54 G 12 = G 13 = 7 GPa, G 23 = 3.7 GPa ρ = 1,600 kg/m 3 1 m 0.4 m Polypropylene foam: E = 0.3 GPa, ν = 0.43 ρ = 400 kg/m 3 Figure 1. Geometry, material and loading for the composite panel. The top and bottom surfaces have four plies of unidirectional carbon/epoxy, each with a thickness of m. The core is made of polypropylene foam. The thickness of the foam is 0.04 m, while the total thickness of the carbon/epoxy lamina is m for the section on both the top and bottom (this makes the panel a total of 0.05 m thick). Mathematical Idealization: Mathematical Representation The foam is too thick to model with shells, thus 3D solid elements must be used. The carbon/epoxy sections are very thin, so they will be modeled with shells. Geometrical Representation Perfect bonding between the foam and the laminates will be assumed, so skinning will be used to section the geometry. Boundary Conditions One side is fixed, and a load is applied to one of the free corners. This induces both a bending moment and torsion in the panel. 2

3 Material Model The foam is linearly elastic, homogeneous and isotropic. The laminate is orthotropic, and linearly elastic. The individual constituents (carbon fibers and epoxy) of the laminate are homogeneous, but the laminate itself is not. Analysis Procedure: 1. Create a new part. It should be a 3D, deformable part, created by Solid Extrusion. 2. Sketch a rectangle with height 0.4 m and length 1 m. 3. Assign an extrusion thickness of 0.04 m. 4. Partition the top face using the Partition Face: Sketch tool. a. Create two sides of a square in the bottom right corner of the face. They should have a side length of 0.05 m. When finished, the part should look like Figure 2. Be sure the long side is aligned with the 1-direction. Figure 2. Plate after part creation and partitioning. 3

4 5. In the Property Module, create a material called Comp_Carbon_Epoxy. Create a density property, and an elastic property. For the latter, change the type to Engineering Constants. Enter the data as shown in Figure Create a second material called Polyprop Foam. Create both a density and an elastic property, as in previous labs for LEHI materials. Enter the data shown in Figure Next, the part will be skinned. The important consequence of this is that when meshed, the part has solid elements and shell elements that share the same nodes. This enforces the same displacement at the boundary of the foam and lamina, which agrees with the perfect bonding assumption made earlier. a. Choose the Create skin tool. Choose the top surface, including the partitioned region. Click Done. b. Choose the bottom surface. Click Done. The top and bottom surfaces have now been skinned. 8. Create a solid, homogeneous section for the foam. 9. Assign the section to the plate. 10. Choose the Create Composite Layup tool. Use a conventional shell with 4 plies. Name it CompositeLayup-Top. Create a layup the same as that shown in Figure 3. a. To choose the region for each ply, double click in the corresponding box. b. Click on the Show/Hide selection options button. c. Change the Select from box to Skins. d. Select the top surface. 4

5 Figure 3. Layup for top surface. 11. On the Offset tab, choose the Bottom Surface radio button. By default, Abaqus puts half the thickness of shell elements above and below the actual elements. In this case, the thickness should all be above the surface for the top layer, and below the surface for the bottom layer. 12. Create another layup, called CompositeLayup-Bottom. It should be very similar to the first layup, but the plies are in reverse order, as shown in Figure 4. Remember to choose the bottom skin for the region. 5

6 Figure 4. Layup for bottom surface. 13. On the Offset tab, choose the Top Surface radio button. Once this is finished, the property definition and assignment is complete. 14. Create an instance of the part in the assembly. 15. Create a Static, Linear Perturbation step. 16. In the field output requests, be sure the strain ( E ) is requested. 17. In the load module, create a boundary condition on the back face that constrains all 6 DOF (U1 = U2 = U3 = UR1 = UR2 = UR3 = 0). 18. Create a pressure load on the partitioned region of the plate with magnitude 4 MPa. This is to apply the 10,000 N load over a small area to prevent stress concentrations. After steps 15 and 16 are complete, the part will look like Figure 5. 6

7 Figure 5. Plate with boundary conditions applied. 19. In the mesh module, apply a global mesh seed of In mesh controls, mesh with Hex elements, and use the Advancing Front algorithm with mapped meshing where appropriate turned on. 21. Assign an element type of C3D8 to the solid region. Assign an element type of S4 to the skinned regions. For the latter, you will need to use the same procedure as for assigning the regions during the layup defintion. 22. Mesh the plate. 23. Create a job, and run the analysis. View the layup orientations and thicknesses. 1. Start in the Property module. 2. Choose Tools Query Ply Stack Plot 3. Choose the surface you wish to view (you will need to choose Skins from the selection filter). 7

8 In this procedure, a layup with orientations [0/90/45/-45] on top and [-45/45/90/0] on bottom was used (Layup #1, below). Analyze the plate with Layup #2 and Layup #3, listed below. It may be useful give each of these a different input deck name. Note the report requirements. 1. [0/90/45/-45] on top and [-45/45/90/0] on bottom 2. [-35/-35/45/0] on top and [0/45/-35/-35] on bottom 3. [10/0/90/-15] on top and [25/0/0/-35] on bottom Model Validation: Set all the plies to have an orientation of 0. Compare the deflection of the plate (average the deflection of the free corners on the bottom surface) to that of a uniform LEHI cantilevered beam with E = E 1. The beam should have a moment of inertia equal to that of the plate, neglecting the stiffness of the foam, but not the position of the laminates. Since the plate does not meet the all the requirements of beam theory (width << length is not true here) there will not be great agreement between the FEA and hand calculations. An order of magnitude comparison is really all that can be drawn from this calculation. If you can find an analytical solution for a plate with these boundary conditions, then a better comparison could be made. Report Requirements: A full report is required for this lab (see ME 475 Lab Report Format Guidelines). Include the following in your report: 1. A plot of the deformed plate with Max Principal strain contours displayed for the layup used in the procedure (Layup #1). 2. Plots of the ply stack plot for Layup #1 (top and bottom surfaces). 3. A plot of the deformed plate with Max Principal strain contours displayed for Layup #2. 4. Plots of the ply stack plot for Layup #2 (top and bottom surfaces). 5. A plot of the deformed plate with Max Principal strain contours displayed for Layup #3. 6. Plots of the ply stack plot for Layup #3 (top and bottom surfaces). 7. Report the maximum principal strain for each of the layups analyzed. 8. Report the maximum z-component of displacement (U3) of the plate for each of the layups analyzed. 8

ME Optimization of a Frame

ME Optimization of a Frame ME 475 - Optimization of a Frame Analysis Problem Statement: The following problem will be analyzed using Abaqus. 4 7 7 5,000 N 5,000 N 0,000 N 6 6 4 3 5 5 4 4 3 3 Figure. Full frame geometry and loading

More information

ME Optimization of a Truss

ME Optimization of a Truss ME 475 - Optimization of a Truss Analysis Problem Statement: The following problem will be analyzed using Abaqus and optimized using HEEDS. 4 5 8 2 11 3 10 6 9 1 7 12 6 m 300 kn 300 kn 22 m 35 m Figure

More information

Simulation of fiber reinforced composites using NX 8.5 under the example of a 3- point-bending beam

Simulation of fiber reinforced composites using NX 8.5 under the example of a 3- point-bending beam R Simulation of fiber reinforced composites using NX 8.5 under the example of a 3- point-bending beam Ralph Kussmaul Zurich, 08-October-2015 IMES-ST/2015-10-08 Simulation of fiber reinforced composites

More information

Chapter 3 Analysis of Original Steel Post

Chapter 3 Analysis of Original Steel Post Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part

More information

MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook

MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook P3*V8.0*Z*Z*Z*SM-PAT325-WBK - 1 - - 2 - Table of Contents Page 1 Composite Model of Loaded Flat Plate 2 Failure Criteria for Flat Plate 3 Making Plies

More information

Laminates can be classified according to the fiber orientation.

Laminates can be classified according to the fiber orientation. Laminates Definition A laminate is an assemblage of individual lamina or plies bonded together normal to their principal plane (i.e., plies are stacked and bonded in their thickness direction). Laminates

More information

A MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun 1

A MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun 1 21 st International Conference on Composite Materials Xi an, 20-25 th August 2017 A MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun

More information

Torsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10

Torsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10 Torsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10 This document contains an Abaqus tutorial for performing a buckling analysis using the finite element program

More information

Introduction to Abaqus. About this Course

Introduction to Abaqus. About this Course Introduction to Abaqus R 6.12 About this Course Course objectives Upon completion of this course you will be able to: Use Abaqus/CAE to create complete finite element models. Use Abaqus/CAE to submit and

More information

Abaqus CAE Tutorial 6: Contact Problem

Abaqus CAE Tutorial 6: Contact Problem ENGI 7706/7934: Finite Element Analysis Abaqus CAE Tutorial 6: Contact Problem Problem Description In this problem, a segment of an electrical contact switch (steel) is modeled by displacing the upper

More information

FINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN

FINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN NAFEMS WORLD CONGRESS 2013, SALZBURG, AUSTRIA FINITE ELEMENT ANALYSIS OF A COMPOSITE CATAMARAN Dr. C. Lequesne, Dr. M. Bruyneel (LMS Samtech, Belgium); Ir. R. Van Vlodorp (Aerofleet, Belgium). Dr. C. Lequesne,

More information

Abaqus-SwiftComp GUI

Abaqus-SwiftComp GUI Abaqus-SwiftComp GUI Version 1.2.2 User s Manual April 21, 2017 Bo Peng Su Tian Lingxuan Zhou Wenbin Yu ii Table of Contents 1 GENERAL INFORMATION...3 1.1 Installation and Get Started...3 1.2 Abaqus-SwiftComp

More information

CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force

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

More information

Modelling Flat Spring Performance Using FEA

Modelling Flat Spring Performance Using FEA Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper

More information

CE366/ME380 Finite Elements in Applied Mechanics I Fall 2007

CE366/ME380 Finite Elements in Applied Mechanics I Fall 2007 CE366/ME380 Finite Elements in Applied Mechanics I Fall 2007 FE Project 1: 2D Plane Stress Analysis of acantilever Beam (Due date =TBD) Figure 1 shows a cantilever beam that is subjected to a concentrated

More information

EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY

EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY J. Sauvé 1*, M. Dubé 1, F. Dervault 2, G. Corriveau 2 1 Ecole de technologie superieure, Montreal, Canada 2 Airframe stress, Advanced Structures,

More information

Revised Sheet Metal Simulation, J.E. Akin, Rice University

Revised Sheet Metal Simulation, J.E. Akin, Rice University Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.

More information

Abaqus/CAE (ver. 6.10) Stringer Tutorial

Abaqus/CAE (ver. 6.10) Stringer Tutorial Abaqus/CAE (ver. 6.10) Stringer Tutorial Problem Description A table made of steel tubing with a solid steel top and shelf is loaded with an oblique impulse load. Determine the transient response of the

More information

NUMERICAL DESIGN OPTIMISATION OF A COMPOSITE REACTION LINK

NUMERICAL DESIGN OPTIMISATION OF A COMPOSITE REACTION LINK THE 19 TH INTERNATIONAL CONFERENCE ON COMPOSITE MATERIALS NUMERICAL DESIGN OPTIMISATION OF A COMPOSITE REACTION LINK Y. Yang*, C. Schuhler, T. London, C. Worrall TWI Ltd, Granta Park, Cambridge CB21 6AL

More information

Workshop 15. Single Pass Rolling of a Thick Plate

Workshop 15. Single Pass Rolling of a Thick Plate Introduction Workshop 15 Single Pass Rolling of a Thick Plate Rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for further processing. The rolling process

More information

ABAQUS/CAE Tutorial: Large Deformation Analysis of Beam-Plate in Bending

ABAQUS/CAE Tutorial: Large Deformation Analysis of Beam-Plate in Bending H. Kim 2004 1 ABAQUS/CAE Tutorial: Large Deformation Analysis of Beam-Plate in Bending Hyonny Kim September 28, 2004 In this tutorial, you ll learn how to: Create a 3D model using shell elements. Conduct

More information

Application of Shell elements to buckling-analyses of thin-walled composite laminates

Application of Shell elements to buckling-analyses of thin-walled composite laminates Application of Shell elements to buckling-analyses of thin-walled composite laminates B.A. Gӧttgens MT 12.02 Internship report Coach: Dr. R. E. Erkmen University of Technology Sydney Department of Civil

More information

OPTFAIL Manual. A1.1 Introduction. APPENDIX 1 SPROPS, PROFAIL, and

OPTFAIL Manual. A1.1 Introduction. APPENDIX 1 SPROPS, PROFAIL, and APPENDIX 1 SPROPS, PROFAIL, and OPTFAIL Manual A1.1 Introduction OPTFAIL is a computer code written in FORTRAN developed by Woodson (1994) to optimize circular frames laminated from uniaxial tape composites

More information

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 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

More information

Learning Module 8 Shape Optimization

Learning Module 8 Shape Optimization Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with

More information

ME 475 Modal Analysis and Optimization of a Tapered Beam

ME 475 Modal Analysis and Optimization of a Tapered Beam ME 475 Modal Analysis and Optimization of a Tapered Beam Objectives: To optimize the shape of a tapered beam to minimize the mass, while holding the first three natural frequencies above those of the baseline

More information

Validation Report: Additional Data Mapping to Structural Analysis Packages

Validation Report: Additional Data Mapping to Structural Analysis Packages Autodesk Moldflow Structural Alliance 2012 Validation Report: Additional Data Mapping to Structural Analysis Packages Mapping process-induced stress data from Autodesk Moldflow Insight Dual Domain and

More information

Guidelines for proper use of Plate elements

Guidelines for proper use of Plate elements Guidelines for proper use of Plate elements In structural analysis using finite element method, the analysis model is created by dividing the entire structure into finite elements. This procedure is known

More information

A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections

A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake

More information

IN-PLANE MATERIAL CONTINUITY FOR THE DISCRETE MATERIAL OPTIMIZATION METHOD

IN-PLANE MATERIAL CONTINUITY FOR THE DISCRETE MATERIAL OPTIMIZATION METHOD IN-PLANE MATERIAL CONTINUITY FOR THE DISCRETE MATERIAL OPTIMIZATION METHOD René Sørensen1 and Erik Lund2 1,2 Department of Mechanical and Manufacturing Engineering, Aalborg University Fibigerstraede 16,

More information

CE Advanced Structural Analysis. Lab 4 SAP2000 Plane Elasticity

CE Advanced Structural Analysis. Lab 4 SAP2000 Plane Elasticity Department of Civil & Geological Engineering COLLEGE OF ENGINEERING CE 463.3 Advanced Structural Analysis Lab 4 SAP2000 Plane Elasticity February 27 th, 2013 T.A: Ouafi Saha Professor: M. Boulfiza 1. Rectangular

More information

Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE

Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE Getting Started with Abaqus: Interactive Edition Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE The following section is a basic tutorial for the experienced Abaqus user. It leads you

More information

FEA of Composites Classical Lamination Theory Example 1

FEA of Composites Classical Lamination Theory Example 1 FEA of Composites Classical Lamination Theory Example 1 22.514 Instructor: Professor James Sherwood Author: Dimitri Soteropoulos Revised by Jacob Wardell Problem Description: A four layer [0/90] s graphite-epoxy

More information

Pro MECHANICA STRUCTURE WILDFIRE 4. ELEMENTS AND APPLICATIONS Part I. Yves Gagnon, M.A.Sc. Finite Element Analyst & Structural Consultant SDC

Pro MECHANICA STRUCTURE WILDFIRE 4. ELEMENTS AND APPLICATIONS Part I. Yves Gagnon, M.A.Sc. Finite Element Analyst & Structural Consultant SDC Pro MECHANICA STRUCTURE WILDFIRE 4 ELEMENTS AND APPLICATIONS Part I Yves Gagnon, M.A.Sc. Finite Element Analyst & Structural Consultant SDC PUBLICATIONS Schroff Development Corporation www.schroff.com

More information

Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses

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,

More information

Finite Element Analysis of a Sandwich Composite Bicycle Frame

Finite Element Analysis of a Sandwich Composite Bicycle Frame 1 Finite Element Analysis of a Sandwich Composite Bicycle Frame Andrew L. Hastert, Benjamin F. Barger, and Justin T. Wood Abstract When designing human-powered transportation vehicles like bicycles, given

More information

Installation Guide. Beginners guide to structural analysis

Installation Guide. Beginners guide to structural analysis Installation Guide To install Abaqus, students at the School of Civil Engineering, Sohngaardsholmsvej 57, should log on to \\studserver, whereas the staff at the Department of Civil Engineering should

More information

Introduction to the Finite Element Method (3)

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

More information

Analysis of Composite Aerospace Structures Finite Elements Professor Kelly

Analysis of Composite Aerospace Structures Finite Elements Professor Kelly Analysis of Composite Aerospace Structures Finite Elements Professor Kelly John Middendorf #3049731 Assignment #3 I hereby certify that this is my own and original work. Signed, John Middendorf Analysis

More information

Top Layer Subframe and Node Analysis

Top Layer Subframe and Node Analysis Top Layer Subframe and Node Analysis By Paul Rasmussen 2 August, 2012 Introduction The top layer of the CCAT backing structure forms a critical interface between the truss and the primary subframes. Ideally

More information

FB-MULTIPIER vs ADINA VALIDATION MODELING

FB-MULTIPIER vs ADINA VALIDATION MODELING FB-MULTIPIER vs ADINA VALIDATION MODELING 1. INTRODUCTION 1.1 Purpose of FB-MultiPier Validation testing Performing validation of structural analysis software delineates the capabilities and limitations

More information

Modeling and Simulation for Aircraft Structural Repair Using Modern FEA Tools

Modeling and Simulation for Aircraft Structural Repair Using Modern FEA Tools Modeling and Simulation for Aircraft Structural Repair Using Modern FEA Tools December 19-22, 2011 and January 9-12, 2012 Kuang-Hua Chang, Ph.D. Williams Presidential Professor School of Aerospace and

More information

Offshore Platform Fluid Structure Interaction (FSI) Simulation

Offshore Platform Fluid Structure Interaction (FSI) Simulation Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,

More information

Efficient Beam-Type Structural Modeling of Rotor Blades

Efficient Beam-Type Structural Modeling of Rotor Blades Downloaded from orbit.dtu.dk on: Dec 8, 28 Efficient Beam-Type Structural Modeling of Rotor Blades Couturier, Philippe; Krenk, Steen Published in: Proceedings of the EWEA Annual Event and Exhibition 25

More information

CHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA

CHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation

More information

Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam

Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam Problem Specification Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam Consider the beam in the figure below. It is clamped on the left side and has a point force of 8kN acting

More information

Abaqus/CAE Axisymmetric Tutorial (Version 2016)

Abaqus/CAE Axisymmetric Tutorial (Version 2016) Abaqus/CAE Axisymmetric Tutorial (Version 2016) Problem Description A round bar with tapered diameter has a total load of 1000 N applied to its top face. The bottom of the bar is completely fixed. Determine

More information

EXPERIMENTAL VALIDATION OF COMPOSITE MATERIAL STRUCTURE OPTIMISATION BY GENETIC ALGORITHM

EXPERIMENTAL VALIDATION OF COMPOSITE MATERIAL STRUCTURE OPTIMISATION BY GENETIC ALGORITHM ICCM11 B043 1 EXPERIMENTAL VALIDATION OF COMPOSITE MATERIAL STRUCTURE OPTIMISATION BY GENETIC ALGORITHM A. Faye (1), B. Paluch (1), M. Grédiac (2) (1) Office National d Etudes et de Recherches Aérospatiales

More information

Multi-Step Analysis of a Cantilever Beam

Multi-Step Analysis of a Cantilever Beam LESSON 4 Multi-Step Analysis of a Cantilever Beam LEGEND 75000. 50000. 25000. 0. -25000. -50000. -75000. 0. 3.50 7.00 10.5 14.0 17.5 21.0 Objectives: Demonstrate multi-step analysis set up in MSC/Advanced_FEA.

More information

ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis

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

More information

Optimal sensor distribution for impact loading identification

Optimal sensor distribution for impact loading identification 11th European Conference on Non-Destructive Testing (ECNDT 2014), October 6-10, 2014, Prague, Czech Republic Optimal sensor distribution for impact loading identification More Info at Open Access Database

More information

Module 1.5: Moment Loading of a 2D Cantilever Beam

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

More information

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 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

More information

Creating and Analyzing a Simple Model in Abaqus/CAE

Creating and Analyzing a Simple Model in Abaqus/CAE Appendix B: Creating and Analyzing a Simple Model in Abaqus/CAE The following section is a basic tutorial for the experienced Abaqus user. It leads you through the Abaqus/CAE modeling process by visiting

More information

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they

More information

Linear and Nonlinear Analysis of a Cantilever Beam

Linear and Nonlinear Analysis of a Cantilever Beam LESSON 1 Linear and Nonlinear Analysis of a Cantilever Beam P L Objectives: Create a beam database to be used for the specified subsequent exercises. Compare small vs. large displacement analysis. Linear

More information

The Mechanics of Composites Collection Material Minds Software A Product of Materials Sciences Corporation

The Mechanics of Composites Collection Material Minds Software A Product of Materials Sciences Corporation The Mechanics of Composites Collection Material Minds Software A Product of Materials Sciences Corporation aterial inds Software The Materials Minds Philosophy Engineers are smart people that want the

More information

Creo Simulate 3.0 Tutorial

Creo Simulate 3.0 Tutorial Creo Simulate 3.0 Tutorial Structure and Thermal Roger Toogood, Ph.D., P. Eng. SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

ANSYS Workbench Guide

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

More information

Exercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0

Exercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0 Exercise 1 3-Point Bending Using the Static Structural Module of Contents Ansys Workbench 14.0 Learn how to...1 Given...2 Questions...2 Taking advantage of symmetries...2 A. Getting started...3 A.1 Choose

More information

FINITE ELEMENT ANALYSIS OF COMPOSITE BOATS

FINITE ELEMENT ANALYSIS OF COMPOSITE BOATS High Performance Yacht Design Conference Auckland, 4-6 December,2002 FINITE ELEMENT ANALYSIS OF COMPOSITE BOATS Don Campbell 1, don@matrix.co.nz Brian Jones 2, brianj@highmodulus.co.nz Abstract. Advances

More information

Prescribed Deformations

Prescribed Deformations u Prescribed Deformations Outline 1 Description 2 Finite Element Model 2.1 Geometry Definition 2.2 Properties 2.3 Boundary Conditions 2.3.1 Constraints 2.3.2 Prescribed Deformation 2.4 Loads 2.4.1 Dead

More information

Module 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis

Module 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis 25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load

More information

1.992, 2.993, 3.04, 10.94, , Introduction to Modeling and Simulation Prof. F.-J. Ulm Spring FE Modeling Example Using ADINA

1.992, 2.993, 3.04, 10.94, , Introduction to Modeling and Simulation Prof. F.-J. Ulm Spring FE Modeling Example Using ADINA 1.992, 2.993, 3.04, 10.94, 18.996, 22.091 Introduction to Modeling and Simulation Prof. F.-J. Ulm Spring 2002 FE Modeling Example Using ADINA H Hgρ w ργ H = B = 10 m g = 9.81 m/s 2 ρ = 2400 kg/m 3 ρ w

More information

Tutorial 10: Composite impact using multi-layered shell elements

Tutorial 10: Composite impact using multi-layered shell elements Tutorial 10 Impact of a Composite Disc using Multilayered Shell Elements Problem description Outline Analysis type(s): Element type(s): Materials law(s): Model options: Key results: Prepared by: Date:

More information

This tutorial will take you all the steps required to set up and run a basic simulation using ABAQUS/CAE and visualize the results;

This tutorial will take you all the steps required to set up and run a basic simulation using ABAQUS/CAE and visualize the results; ENGN 1750: Advanced Mechanics of Solids ABAQUS TUTORIAL School of Engineering Brown University This tutorial will take you all the steps required to set up and run a basic simulation using ABAQUS/CAE and

More information

Introduction to Finite Element Analysis using ANSYS

Introduction to Finite Element Analysis using ANSYS Introduction to Finite Element Analysis using ANSYS Sasi Kumar Tippabhotla PhD Candidate Xtreme Photovoltaics (XPV) Lab EPD, SUTD Disclaimer: The material and simulations (using Ansys student version)

More information

Module 1.6: Distributed Loading of a 2D Cantilever Beam

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

More information

Exercise 1: 3-Pt Bending using ANSYS Workbench

Exercise 1: 3-Pt Bending using ANSYS Workbench Exercise 1: 3-Pt Bending using ANSYS Workbench Contents Starting and Configuring ANSYS Workbench... 2 1. Starting Windows on the MAC... 2 2. Login into Windows... 2 3. Start ANSYS Workbench... 2 4. Configuring

More information

Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole

Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole Problem Specification Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole Consider the classic example of a circular hole in a rectangular plate of constant thickness. The plate

More information

Targeting Composite Wing Performance Optimising the Composite Lay-Up Design

Targeting Composite Wing Performance Optimising the Composite Lay-Up Design Targeting Composite Wing Performance Optimising the Composite Lay-Up Design Sam Patten Optimisation Specialist, Altair Engineering Ltd Imperial House, Holly Walk, Royal Leamington Spa, CV32 4JG sam.patten@uk.altair.com

More information

SIMULATION CAPABILITIES IN CREO

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

More information

Abaqus CAE Tutorial 1: 2D Plane Truss

Abaqus CAE Tutorial 1: 2D Plane Truss ENGI 7706/7934: Finite Element Analysis Abaqus CAE Tutorial 1: 2D Plane Truss Lab TA: Xiaotong Huo EN 3029B xh0381@mun.ca Download link for Abaqus student edition: http://academy.3ds.com/software/simulia/abaqus-student-edition/

More information

This tutorial will take you all the steps required to import files into ABAQUS from SolidWorks

This tutorial will take you all the steps required to import files into ABAQUS from SolidWorks ENGN 1750: Advanced Mechanics of Solids ABAQUS CAD INTERFACE TUTORIAL School of Engineering Brown University This tutorial will take you all the steps required to import files into ABAQUS from SolidWorks

More information

An Overview of Computer Aided Design and Finite Element Analysis

An Overview of Computer Aided Design and Finite Element Analysis An Overview of Computer Aided Design and Finite Element Analysis by James Doane, PhD, PE Contents 1.0 Course Overview... 4 2.0 General Concepts... 4 2.1 What is Computer Aided Design... 4 2.1.1 2D verses

More information

Predicting the mechanical behaviour of large composite rocket motor cases

Predicting the mechanical behaviour of large composite rocket motor cases High Performance Structures and Materials III 73 Predicting the mechanical behaviour of large composite rocket motor cases N. Couroneau DGA/CAEPE, St Médard en Jalles, France Abstract A method to develop

More information

Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench

Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench Contents Beam under 3-Pt Bending [Balken unter 3-Pkt-Biegung]... 2 Taking advantage of symmetries... 3 Starting and Configuring ANSYS Workbench... 4 A. Pre-Processing:

More information

Embedded Reinforcements

Embedded Reinforcements Embedded Reinforcements Gerd-Jan Schreppers, January 2015 Abstract: This paper explains the concept and application of embedded reinforcements in DIANA. Basic assumptions and definitions, the pre-processing

More information

Inspection of Spar-Core Bond in Helicopter Rotor Blades Using Finite Element Analysis

Inspection of Spar-Core Bond in Helicopter Rotor Blades Using Finite Element Analysis Inspection of Spar-Core Bond in Helicopter Rotor Blades Using Finite Element Analysis Sunil Kishore Chakrapani* a,b, Daniel J. Barnard a, and Vinay Dayal a,b a Center for NDE, Iowa State University, Ames,

More information

Finite Element Analysis Using Creo Simulate 4.0

Finite Element Analysis Using Creo Simulate 4.0 Introduction to Finite Element Analysis Using Creo Simulate 4.0 Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

Introduction to Nastran SOL 200 Design Sensitivity and Optimization

Introduction to Nastran SOL 200 Design Sensitivity and Optimization Introduction to Nastran SOL 200 Design Sensitivity and Optimization PRESENTED BY: CHRISTIAN APARICIO The Nastran Engineering SOL 200 questions? Lab Email me: christian@ the-engineering-lab.com Motivation

More information

CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1

CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Outcome 1 The learner can: CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Calculate stresses, strain and deflections in a range of components under

More information

Performance Evaluation of Finite Elements for Analysis of Advanced Hybrid Laminates

Performance Evaluation of Finite Elements for Analysis of Advanced Hybrid Laminates Performance Evaluation of Finite Elements for Analysis of Advanced Hybrid Laminates Hemanth R. H, Ruchin P, Gourav G, Venkatesha K. S and Ravi Kumar, G. V. V Infosys Technologies Limited, Electronic City,

More information

ANSYS AIM Tutorial Structural Analysis of a Plate with Hole

ANSYS AIM Tutorial Structural Analysis of a Plate with Hole ANSYS AIM Tutorial Structural Analysis of a Plate with Hole Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Analytical vs. Numerical Approaches

More information

3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation

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

More information

Using Abaqus to Model Delamination in Fiber- Reinforced Composite Materials

Using Abaqus to Model Delamination in Fiber- Reinforced Composite Materials Using Abaqus to Model Delamination in Fiber- Reinforced Composite Materials Dimitri Soteropoulos, Konstantine A. Fetfatsidis and James A. Sherwood Department of Mechanical Engineering, University of Massachusetts

More information

Finite Element Analysis Using NEi Nastran

Finite Element Analysis Using NEi Nastran Appendix B Finite Element Analysis Using NEi Nastran B.1 INTRODUCTION NEi Nastran is engineering analysis and simulation software developed by Noran Engineering, Inc. NEi Nastran is a general purpose finite

More information

Investigation of Structural Behavior due to. Bend-Twist Couplings in Wind Turbine Blades

Investigation of Structural Behavior due to. Bend-Twist Couplings in Wind Turbine Blades Investigation of Structural Behavior due to Bend-Twist Couplings in Wind Turbine Blades V.A. Fedorov* 1, N. Dimitrov*, C. Berggreen*, S. Krenk*, K. Branner and P. Berring * Department of Mechanical Engineering,

More information

Manual for Computational Exercises

Manual for Computational Exercises Manual for the computational exercise in TMM4160 Fracture Mechanics Page 1 of 32 TMM4160 Fracture Mechanics Manual for Computational Exercises Version 3.0 Zhiliang Zhang Dept. of Structural Engineering

More information

ECE421: Electronics for Instrumentation

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

More information

Finite Element Method. Chapter 7. Practical considerations in FEM modeling

Finite Element Method. Chapter 7. Practical considerations in FEM modeling Finite Element Method Chapter 7 Practical considerations in FEM modeling Finite Element Modeling General Consideration The following are some of the difficult tasks (or decisions) that face the engineer

More information

COMSOL BASED 2-D FEM MODEL FOR ULTRASONIC GUIDED WAVE PROPAGATION IN SYMMETRICALLY DELAMINATED UNIDIRECTIONAL MULTI- LAYERED COMPOSITE STRUCTURE

COMSOL BASED 2-D FEM MODEL FOR ULTRASONIC GUIDED WAVE PROPAGATION IN SYMMETRICALLY DELAMINATED UNIDIRECTIONAL MULTI- LAYERED COMPOSITE STRUCTURE Proceedings of the National Seminar & Exhibition on Non-Destructive Evaluation NDE 2011, December 8-10, 2011 COMSOL BASED 2-D FEM MODEL FOR ULTRASONIC GUIDED WAVE PROPAGATION IN SYMMETRICALLY DELAMINATED

More information

FDM Lightweight Structures DESIGN GUIDE

FDM Lightweight Structures DESIGN GUIDE FDM Lightweight Structures THE 3D PRINTING SOLUTIONS COMPANY FDM Lightweight Structures Many aerospace and automotive applications require parts with a very high stiffness-to-weight ratio. Because of the

More information

4-2 Quasi-Static Fatigue

4-2 Quasi-Static Fatigue 1 4-2 Quasi-Static Fatigue Case Description: Example Location: Composite coupon subject to tensile cyclic loading Tutorials > Fatigue > Quasi Static Fatigue Model Description: Nodes: 261; Elements: 224

More information

Computations of stresses with volume-elements in rectangular and HE sections

Computations of stresses with volume-elements in rectangular and HE sections CT3000: Bachelor Thesis Report, Izik Shalom (4048180) Computations of stresses with volume-elements in rectangular and HE sections Supervisors: dr. ir. P.C.J. Hoogenboom en Ir. R. Abspoel June 2013 Preface

More information

2: Static analysis of a plate

2: Static analysis of a plate 2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors

More information

NonLinear Analysis of a Cantilever Beam

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

More information

ENGINEERING TRIPOS PART IIA FINITE ELEMENT METHOD

ENGINEERING TRIPOS PART IIA FINITE ELEMENT METHOD ENGINEERING TRIPOS PART IIA LOCATION: DPO EXPERIMENT 3D7 FINITE ELEMENT METHOD Those who have performed the 3C7 experiment should bring the write-up along to this laboratory Objectives Show that the accuracy

More information

Buckling Analysis of a Thin Plate

Buckling Analysis of a Thin Plate Buckling Analysis of a Thin Plate Outline 1 Description 2 Modeling approach 3 Finite Element Model 3.1 Units 3.2 Geometry definition 3.3 Properties 3.4 Boundary conditions 3.5 Loads 3.6 Meshing 4 Structural

More information

MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1

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

More information