CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
|
|
- Buddy Pope
- 6 years ago
- Views:
Transcription
1 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 boundary conditions, element types, validation, and the force distribution collection methods are discussed. Optimization measures of the numerical models are also included in this chapter. The finite element software used in the development of the numerical models is I-DEAS Master Series 9m3 [30]. The relatively robust and user-friendly solid modeling and finite element meshing interface are the main advantages of this solid modeling/ finite element software. 4.1 Model Assumptions All the numerical analyses done in this research involves the use of non-linear analysis capability of I-DEAS, including geometric non-linearity and material nonlinearity. With geometric non-linearity, the software takes the effect of shape change into account while calculating the solution. Using material non-linearity the non-linear behavior of the material response (i.e. post yield material properties) is taken into account. It is important to compare and contrast the assumptions made by the theoretical and numerical models in order to achieve meaningful comparisons. Below are the assumptions made for the numerical models: 1. Face sheets and core are perfectly bonded 52
2 The numerical model assumes no delamination occur between layers. This assumption is consistent with the assumptions made in the classical sandwich plate theory and higher order theory. 2. Face sheets remain elastic at all time Due to the significantly higher yield strength and modulus of elasticity of the face sheets compared to the core, face sheets are assumed to remain elastic throughout the loading for both the four-point bend test and HTS. This assumption is also consistent with the assumptions made in the classical sandwich plate theory and higher order theory 3. Load scenarios are quasi-static The two load cases considered were modeled quasi-statically instead of dynamically. Incremental loadings are applied slowly during the actual experiments. Therefore, the type of analyses done for this research effort is called static, non-linear analysis. 4. Geometric non-linearity has a significant effect Geometric non-linearity is considered to have significant effect on the load distribution on each layer of the sandwich structure. Therefore all the numerical analyses done take geometric non-linearity into consideration. This is the main difference between the numerical models and the theoretical models. Classical sandwich plate theory and higher order theory do not take shape change of the sandwich structures into account. 53
3 4.2 Four-point Bend Test Numerical Model The sandwich structure in the four-point bend test model had Aluminum T3 face sheets and a Herex C foam core as stated in chapter three. The beam model was partitioned into three layers, forming three perfectly bonded material layers Boundary Conditions/ Mesh Due to the symmetric nature of the problem, only half of the beam was modeled. The boundary conditions applied to the half beam model are shown in Figure 4.1. The beam has a roller support. Thus the left support of the model is given translational freedom in the X-direction and rotational freedom about the Z-axis. The vertical lines in Figure 4.1 show the partitions made along the beam s length in order to allow element force calculation in the post-processing part of the analysis. Y Region 1 P (Region 13) 2 Region 20 X Roller X translation free Y translation fixed Z rotation free Symmetry X translation fixed Y translation free Z rotation fixed FIGURE 4.1 Sandwich beam boundary conditions and partitions. 54
4 The partitions split the beam into several volumes which were labeled as Region 1 to Region 20 for convenience in data collection from the left to the right boundary. The element force calculation method will be discussed in detail later. A line load is applied to the top edge of Region 13 (Figure 4.1), simulating the load transmitted from the upper rollers to the beam. The beam is loaded with a set of loads that vary slowly with time, and results are calculated at each load step. Figure 4.2 shows the time variation form. FIGURE 4.2 Setting time varying load steps on I-DEAS. The time intervals between load steps are not important because the model is assumed to be quasi-static and the analysis type done is a static analysis. The finite element software was set in such a way that corresponding solutions are completed at 55
5 each load step as shown in Figure 4.3. This allows all the analysis to be done in a single run of the finite element model. As a result, the model would take up less memory space because one single solid model and finite element model can be used for all load steps. FIGURE 4.3 Setting multiple solution points on I-DEAS. The numerical model of the four-point bend test utilizes the mapped mesh capability of I-DEAS. By controlling the number of nodes along each edge of the solid model, this function allows total control of the mesh size. The element size is chosen by referring to Miers [14] work in mesh refinement. Miers [14] recommended a core element size of 1.5 mm and face element size of 3 mm in order to achieve convergence in the data obtained. Constant mesh density is ensured with the mapped meshing function. This is important because constant mesh density ensures that data collected from any region of the beam are of the same degree of resolution. Three-dimensional (solid) brick 56
6 elements are used in this analysis. Second order (parabolic) brick elements are chosen over the first order (linear) brick elements in order to better interpolate the data between nodes. Figure 4.4 shows the meshed model of the sandwich beam with corresponding boundary conditions. FIGURE 4.4 Meshed sandwich beam with boundary conditions. Since the analysis involves material non-linearity, a yield function or yield criteria needs to be defined for the model. Von Mises yield criteria and its associated flow rule are used in this analysis. Isotropic hardening is also used to describe the change of the yield criterion as a result of plastic straining. Only the core elements are assigned a yield function due to the assumption that only core yielding occurs throughout the loading process. The face sheets are assumed to remain elastic at all time, hence no yield function is assigned to the face sheet elements. 57
7 4.2.2 Validation In order to validate the finite element model, the numerically obtained loaddeflection curve is compared with the actual experimental load-deflection curve (Figure 4.5) Load (N) Experimental Numerical Center Beam Deflection (mm) FIGURE 4.5 Comparison of load versus center deflection for four-point bend test. The numerical result shows good correlation with the experimental result. The slight discrepancy is due to the error caused by the material properties that do not fully define the post yield property of the core material. However, this model is sufficient to achieve the purpose of this research, which is to determine the load distribution within the sandwich beam and the effect of geometric non-linearity on this load distribution Element Force Collection In order to calculate the amount of load carried by each layer of the sandwich beam at several locations along the beam s length, the beam is partitioned into twenty 58
8 different portions. Each portion consists of top face sheet, core, and bottom face sheet, thus there are sixty volumes altogether. By utilizing the grouping capability of I-DEAS, specific volumes and finite element entities of interest can be grouped together and analyzed. The grouped model then functions as free body diagrams, allowing the author to find out the load distribution on the regions of interest. For example, as shown in Figure 4.6, the volumes before Region 16 and their related elements and nodes are grouped together. Full Beam Cut Beam Exposed Surface for analysis FIGURE 4.6 Grouped volumes and finite element entities of sandwich beam. By only showing this group of entities, the cross section of Region 16 can be exposed. The element force, stress and strain contour can be analyzed on that specific surface. In order to see the cross sections of all the sixty volumes of the beam model, 59
9 sixty groups were created. The groups were labeled as Core Region 1-20, Top Face Sheet Region 1-20, and Bottom Face Sheet Region The groupings are like making a cut on a free body diagram. The Region 1 cut would consist of the volume prior to Region 1, Region 2 cut would include all the volumes before the Region 2 cross section, and so on. In order to find out the actual load carried by a particular layer (core, top face sheet or bottom face sheet) at any surface of interest, the load carried by each node on that surface needs to be calculated. To achieve this there are three challenges that need to be overcome: 1. Data search from the data pool The element force data associated with each node can be stored in a specific data file using I-DEAS. However, there is a need to extract the element force data that corresponds only to the nodes on the surface of interest. 2. Nodes of interest identification I-DEAS labels each node with a unique node number in order to make each node identifiable. Therefore each node that is on the surface of interest has a unique node number. There is a need to obtain the list of node numbers that corresponds to the nodes on the surface of interest. 3. Distinguish nodes on different material layer surfaces In the list of node numbers of interest collected, the nodes that correspond to each layer (core, top face sheet, or bottom face sheet) needs to be distinguished. The first step to overcome the above-mentioned problems is to collect the node numbers of the nodes on the surface of interest. In order to do this the author used the info function of I-DEAS to list the info of all the nodes on a specific surface. I-DEAS 60
10 allows its users to limit the entity selection. In this case, the author made nodes the only pickable entity. I-DEAS also allows a user to pick entities that are related to certain geometry. Therefore if the surface of interest is the cross section of the top face sheet, users can set the options as pick only nodes and related to surface, and then pick the cross section of the top face sheet. I-DEAS will then list the information about the nodes that are on that selected surface on the I-DEAS List screen (Figure 4.7). FIGURE 4.7 Node information on I-DEAS List window. The information listed including node numbers and their x, y, z-coordinate positions. This list of node information can be copied, pasted and saved on a text editor. Same process would be repeated for the cross section of each layers of each of the twenty regions along the beam, resulting a total of sixty sets of node numbers and locations. The next step is to extract the element force data. Element force data is extracted from the sixty volume groups. Thus there are sixty corresponding element force data files for the sixty groups of the beam. By using the Report Writer function of I- DEAS (Figure 4.8), the element force data can be generated and stored as.dat format. 61
11 FIGURE 4.8 Report writer window. Figure 4.9 shows an example of the element force data file for the region one core, opened using a text editor. The node numbers and element forces are then load and saved in a Matlab file. The information listed on the element force data file are the node numbers, element forces in x, y, and z directions, and moments about x, y, and z-axes. It should be noted that this coordinate system is with respect to the global coordinate system. The importance of this is explained in chapter five. At this point the element force data from the sets of free body diagram cuts and the node numbers sets on the surfaces of interest has been obtained. 62
12 FIGURE 4.9 Element force data file on Text Editor. The final procedure would be to match the node numbers on the surfaces of interest with the element force data files of each group of free body diagram cuts. A Matlab program (appendix A) was written to match the node numbers of a particular surface and extract the corresponding element force values from the corresponding set of element force data. All node forces can then be summed and the resulting load in the x, y, and z directions of a particular surface is obtained. 4.3 Hydromat Test System Numerical Model The sandwich panel used for HTS has 3003-H14 aluminum face sheets and an Airex R63.50 core. Similar to the beam model, the solid model of the sandwich panel subjected to HTS is partitioned into three perfectly bonded layers. 63
13 4.3.1 Boundary Conditions/ Mesh The symmetric nature of the problem allows only a quarter of the whole panel needs to be meshed. The boundary conditions used are shown on Figure Region 1 Region 10 Y X Simply Supported X translation free Z rotation free Symmetry Y translation free Z translation free X rotation free FIGURE 4.10(a) Sandwich panel boundary conditions, X-Y plane. Region 1 Region 10 Y Z Simply Supported Z translation free X rotation free Symmetry Y translation free X translation free Z rotation free FIGURE 4.10(b) Sandwich panel boundary conditions, Y-Z plane. The two planes of symmetry of the panel have symmetric boundary conditions, where in-plane displacements and rotation about an axis respective normal to the symmetry plane is allowed. A simply supported boundary condition is applied to the two 64
14 other edges of the quarter plate. This simulates the simply supported condition of the panel resting on the HTS fixture. A distributed load is applied on the top surface of the sandwich panel, simulating the load transfer from the pressurized bladder to the panel. A step pressure model is used in this simulation. The area in which the distributed load is applied is the effective area obtained using equation In other words, the contact area changes as the applied pressure increases. This approach is consistent with the theoretical model. Table 4.1 shows the corresponding contact area at different load steps analyzed and the total applied load. The effective contact area was obtained from Eyre s [25] work. Table 4.1 HTS loading details. Pressure Effective Contact Area Total Applied Load (kpa) (m 2 ) (kn) The sandwich panel is partitioned into ten different regions that are labeled from Region 1 to Region 10 respectively (Figure 4.10(a), Figure 4.10(b)). Distributed loads are applied beginning from Region 4 to Region 10 (Figure 4.11). The effective contact region is assumed to be a perfectly square shape, therefore the aspect ratio between the length and width of the effective contact area is set as one. This uniform aspect ratio ensures the symmetry nature of the loading scenario and allows analysis done on only a quarter of the plate. 65
15 Region 4 Region 10 FIGURE 4.11 Distributed load applied on the panel top surface. Similar to the four-point bend test model, the elements used in this simulation are three dimensional, parabolic, brick elements. Again the element sizes were chosen according to the recommendation made in Miers [14] work, where a core element size of 1.5 mm and face element size of 3 mm are used. The solid model is meshed using the mapped meshing capability of I-DEAS. The core is assumed to be the only material that undergoes plastic deformation. The core elements use the Von Mises plastic yield function and undergo isotropic hardening Elastic Edge During the analysis, localized core yielding occurs due to the simply supported edges. Although a small region of the core right above the support lines is involved, the deformation in these regions were higher than other regions of the core. At the kpa (15 psi) load step, excessive localized yielding occurs and halted the finite element analysis. In order to bypass this localized yielding problem, the core region that is 66
16 directly above the edge support was made elastic. The elastic edge has the same material properties as the foam core except there is no yield criteria assigned to elements of that region. This prevents the core from yielding at the region close to the support lines without changing the plate response significantly. Validation of this method is shown in the next section. Figure 4.12 shows the full elastic edge used for the kpa load step. The effect of a half elastic edge was also investigated during the validation process. Half elastic edge simply means only the bottom half volumes of the edge is made elastic, and the top half volumes could still undergo plastic deformation. FIGURE 4.12 Full elastic edge (shown in green) used in sandwich core Validation In order to validate the finite element model the load versus center deflection curve obtained from the model is compared with the experimental data. The experimental 67
17 data is obtained from Eyre s [25] work in The numerical model shows good correlation with the experimental results. Error begins to grow as the core yielding begins to take place. This discrepancy is believed to be caused by inaccuracy in post yield material properties Load (N) Experimental Numerical Center Panel Deflection (mm) FIGURE 4.13 Comparison of load versus center panel deflection for HTS. To ensure that the elastic edge added to the core does not alter the overall behavior of the sandwich plate, the 86.2 kpa (12.5 psi) load step was used as a check. The 86.2kPa load scenario was analyzed again for two other conditions, one with a half elastic edge and another with a full elastic edge. The center panel deflection difference between the models with elastic edges and the model without elastic edge were found to be less than 3%. The shear load distributions on each layer of the panel are shown in appendix C. Shear load plots of the three models on each layer of the sandwich panel considered show excellent agreement throughout the plate span. This shows that the elastic edge insert is a viable method and validates the usage of this method for the kpa load step. 68
18 4.3.4 Element Force Collection The force collection procedures used for the HTS numerical model is similar to the four-point bend test numerical model. Load distribution on each layer is collected and summed on each surface of interest. Forces are collected with respect to the global coordinate system. The element forces on each surface of interest are then calculated using a Matlab program. The results obtained are presented in the next chapter. 69
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 informationExample 24 Spring-back
Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static
More informationModule 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 informationExercise 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 informationModule 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 informationThe part to be analyzed is the bracket from the tutorial of Chapter 3.
Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component
More informationNon-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla
Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla 1 Faculty of Civil Engineering, Universiti Teknologi Malaysia, Malaysia redzuan@utm.my Keywords:
More informationModelling 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 informationCOMPUTER 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.
More informationExercise 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 informationSimulation of RF HEat Test
Simulation of RF HEat Test Date: Tuesday, December 22, 2015 Designer: Solidworks Study name: Stress One Third Emissivity Analysis type: Nonlinear - Dynamic Description No Data Table of Contents Description...
More informationChapter 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 informationRevision 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 informationModule 1.3W Distributed Loading of a 1D Cantilever Beam
Module 1.3W Distributed Loading of a 1D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Workbench Analysis System 4 Engineering Data 5 Geometry 6 Model 11 Setup 13 Solution
More informationExercise 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 information3D 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 informationEngineering 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 informationSimulation of AJWSP10033_FOLDED _ST_FR
Phone: 01922 453038 www.hyperon-simulation-and-cad-services.co.uk Simulation of AJWSP10033_FOLDED _ST_FR Date: 06 May 2017 Designer: Study name: AJWSP10033_FOLDED_STATIC Analysis type: Static Description
More informationModule 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
More informationModule 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
More informationGuidelines 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 informationEmbedded 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 informationSome Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact
Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact Eduardo Luís Gaertner Marcos Giovani Dropa de Bortoli EMBRACO S.A. Abstract A linear elastic model is often not appropriate
More informationQuarter Symmetry Tank Stress (Draft 4 Oct 24 06)
Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of
More informationModule 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 informationME 442. Marc/Mentat-2011 Tutorial-1
ME 442 Overview Marc/Mentat-2011 Tutorial-1 The purpose of this tutorial is to introduce the new user to the MSC/MARC/MENTAT finite element program. It should take about one hour to complete. The MARC/MENTAT
More informationAufgabe 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 information2: 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 informationA 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 =
More informationES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010
ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.
More informationSETTLEMENT OF A CIRCULAR FOOTING ON SAND
1 SETTLEMENT OF A CIRCULAR FOOTING ON SAND In this chapter a first application is considered, namely the settlement of a circular foundation footing on sand. This is the first step in becoming familiar
More informationChapter 7 Practical Considerations in Modeling. Chapter 7 Practical Considerations in Modeling
CIVL 7/8117 1/43 Chapter 7 Learning Objectives To present concepts that should be considered when modeling for a situation by the finite element method, such as aspect ratio, symmetry, natural subdivisions,
More informationME 475 FEA of a Composite Panel
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
More informationExercise 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 informationCHAPTER-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 informationInvestigation of the behaviour of single span reinforced concrete historic bridges by using the finite element method
Structural Studies, Repairs and Maintenance of Heritage Architecture XI 279 Investigation of the behaviour of single span reinforced concrete historic bridges by using the finite element method S. B. Yuksel
More informationReinforced concrete beam under static load: simulation of an experimental test
Reinforced concrete beam under static load: simulation of an experimental test analys: nonlin physic. constr: suppor. elemen: bar cl12i cl3cm compos cq16m interf pstres reinfo struct. load: deform weight.
More informationWorkshop 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 informationNEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN
Vol 4 No 3 NEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN Ass Lecturer Mahmoud A Hassan Al-Qadisiyah University College of Engineering hasaaneng@yahoocom ABSTRACT This paper provides some lighting
More informationANSYS 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 informationMSC/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 informationLIGO Scissors Table Static Test and Analysis Results
LIGO-T980125-00-D HYTEC-TN-LIGO-31 LIGO Scissors Table Static Test and Analysis Results Eric Swensen and Franz Biehl August 30, 1998 Abstract Static structural tests were conducted on the LIGO scissors
More informationMulti-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 informationStiffened Plate With Pressure Loading
Supplementary Exercise - 3 Stiffened Plate With Pressure Loading Objective: geometry and 1/4 symmetry finite element model. beam elements using shell element edges. MSC.Patran 301 Exercise Workbook Supp3-1
More informationANSYS 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 informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More informationLOCAL STRESS ANALYSIS OF STIFFENED SHELLS USING MSC/NASTRAN S SHELL AND BEAM p-elements
LOCAL STRESS ANALYSIS OF STIFFENED SHELLS USING MSC/NASTRAN S SHELL AND BEAM p-elements Sanjay Patel, Claus Hoff, Mark Gwillim The MacNeal-Schwendler Corporation Abstract In large finite element models
More informationFE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS
Proceedings of ICAD26 FE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS ICAD-26-43 Enrico Armentani enrico.armentani@unina.it University of Naples P.le V. Tecchio, 8 8125 Naples Italy Francesco
More informationSimilar Pulley Wheel Description J.E. Akin, Rice University
Similar Pulley Wheel Description J.E. Akin, Rice University The SolidWorks simulation tutorial on the analysis of an assembly suggested noting another type of boundary condition that is not illustrated
More informationRecent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA
14 th International LS-DYNA Users Conference Session: Simulation Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA Hailong Teng Livermore Software Technology Corp. Abstract This paper
More informationStep Change in Design: Exploring Sixty Stent Design Variations Overnight
Step Change in Design: Exploring Sixty Stent Design Variations Overnight Frank Harewood, Ronan Thornton Medtronic Ireland (Galway) Parkmore Business Park West, Ballybrit, Galway, Ireland frank.harewood@medtronic.com
More informationModule 1.7W: Point Loading of a 3D Cantilever Beam
Module 1.7W: Point Loading of a 3D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Workbench Analysis System 4 Engineering Data 5 Geometry 6 Model 11 Setup 13 Solution 14 Results
More informationInfluence of geometric imperfections on tapered roller bearings life and performance
Influence of geometric imperfections on tapered roller bearings life and performance Rodríguez R a, Calvo S a, Nadal I b and Santo Domingo S c a Computational Simulation Centre, Instituto Tecnológico de
More informationFinite 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 informationLinear 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 informationTWO-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
More informationTHREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD
THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD Haval Kamal Asker Department of Mechanical Engineering, Faculty of Agriculture and Forestry, Duhok University, Duhok,
More informationFOUNDATION IN OVERCONSOLIDATED CLAY
1 FOUNDATION IN OVERCONSOLIDATED CLAY In this chapter a first application of PLAXIS 3D is considered, namely the settlement of a foundation in clay. This is the first step in becoming familiar with the
More informationCHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS
CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS 7.1 GENERAL An analytical study on behaviour of combined effect of optimised channel sections using ANSYS was carried out and discussed in
More informationElement 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
More informationE and. L q. AE q L AE L. q L
STRUTURL NLYSIS [SK 43] EXERISES Q. (a) Using basic concepts, members towrds local axes is, E and q L, prove that the equilibrium equation for truss f f E L E L E L q E q L With f and q are both force
More informationSettlement of a circular silo foundation
Engineering manual No. 22 Updated: 02/2018 Settlement of a circular silo foundation Program: FEM File: Demo_manual_22.gmk The objective of this manual is to describe the solution to a circular silo foundation
More informationComputer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks
Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Finite Element Analysis of Bearing Box on SolidWorks Chenling Zheng 1, a, Hang Li 1, b and Jianyong Li 1, c 1 Shandong University
More informationNonLinear 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
More informationPLAXIS 2D - SUBMERGED CONSTRUCTION OF AN EXCAVATION
PLAXIS 2D - SUBMERGED CONSTRUCTION OF AN EXCAVATION 3 SUBMERGED CONSTRUCTION OF AN EXCAVATION This tutorial illustrates the use of PLAXIS for the analysis of submerged construction of an excavation. Most
More informationContents Metal Forming and Machining Processes Review of Stress, Linear Strain and Elastic Stress-Strain Relations 3 Classical Theory of Plasticity
Contents 1 Metal Forming and Machining Processes... 1 1.1 Introduction.. 1 1.2 Metal Forming...... 2 1.2.1 Bulk Metal Forming.... 2 1.2.2 Sheet Metal Forming Processes... 17 1.3 Machining.. 23 1.3.1 Turning......
More informationSuper Elastic Alloy Eyeglass Frame Design Using the ANSYS Workbench Environment
Super Elastic Alloy Eyeglass Frame Design Using the ANSYS Workbench Environment Peter R. Barrett, P.E. Computer Aided Engineering Associates Inc. Patrick Cunningham Computer Aided Engineering Associates
More informationA 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 informationVOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL
VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL The following is a description of the model setups and input/output parameters for benchmarking analytical volcanic deformation models
More informationManual 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 informationSimulation of TEST DAVIT
Phone: 616-834-4175 WWW.SKYLINEFP.COM Simulation of TEST DAVIT Date: Friday, February 19, 2016 Designer: Study name: Study 1 Analysis type: Static Description No Data Table of Contents Description... 1
More informationLearning 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 informationAppendix 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 informationSUBMERGED CONSTRUCTION OF AN EXCAVATION
2 SUBMERGED CONSTRUCTION OF AN EXCAVATION This tutorial illustrates the use of PLAXIS for the analysis of submerged construction of an excavation. Most of the program features that were used in Tutorial
More informationCHAPTER 1. Introduction
ME 475: Computer-Aided Design of Structures 1-1 CHAPTER 1 Introduction 1.1 Analysis versus Design 1.2 Basic Steps in Analysis 1.3 What is the Finite Element Method? 1.4 Geometrical Representation, Discretization
More informationFinite Element Specialists and Engineering Consultants
Finite Element Specialists and Engineering Consultants Limit Analysis Using Finite Element Techniques Seminar for the Advanced Structural Engineering Module College of Engineering, Mathematics & Physical
More informationANSYS 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 informationSDC. Engineering Analysis with COSMOSWorks. Paul M. Kurowski Ph.D., P.Eng. SolidWorks 2003 / COSMOSWorks 2003
Engineering Analysis with COSMOSWorks SolidWorks 2003 / COSMOSWorks 2003 Paul M. Kurowski Ph.D., P.Eng. SDC PUBLICATIONS Design Generator, Inc. Schroff Development Corporation www.schroff.com www.schroff-europe.com
More informationAbaqus/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 informationCreo 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 informationInternal Forces and Moments
Introduction Internal Forces and Moments To a very large extend this chapter is simply an extension of Section 6.3, The Method of Sections. The section on curved cables is new material. The section on
More informationComputational Simulation of Cylindrical Pressure Loading
Computational Simulation of Cylindrical Pressure Loading MEG 795 Special Topics: Energy Methods II Presented By: Nallani Gopi Nov 20, 2003 Department of Mechanical Engineering University of Nevada,Las
More informationCrashbox Tutorial. In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0
Crashbox Tutorial In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0 (Written by Moritz Guenther, student at Altair Engineering GmbH) 1 HyperMesh* 1. Start
More informationCE 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 informationAnalysis Steps 1. Start Abaqus and choose to create a new model database
Source: Online tutorials for ABAQUS Problem Description The two dimensional bridge structure, which consists of steel T sections (b=0.25, h=0.25, I=0.125, t f =t w =0.05), is simply supported at its lower
More informationStudy of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket
RESEARCH ARTICLE OPEN ACCESS Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket Gowtham K L*, Shivashankar R. Srivatsa** *(Department of Mechanical Engineering, B. M.
More informationTorsional-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 informationAn 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 informationSliding Split Tube Telescope
LESSON 15 Sliding Split Tube Telescope Objectives: Shell-to-shell contact -accounting for shell thickness. Creating boundary conditions and loads by way of rigid surfaces. Simulate large displacements,
More informationFinite 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 informationWORKSHOP 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.
More informationA Computational Study of Local Stress Intensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens
A Computational Study of Local Stress ntensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens D.-A. Wang a and J. Pan b* a Mechanical & Automation Engineering, Da-Yeh University,
More informationABAQUS for CATIA V5 Tutorials
ABAQUS for CATIA V5 Tutorials AFC V2.5 Nader G. Zamani University of Windsor Shuvra Das University of Detroit Mercy SDC PUBLICATIONS Schroff Development Corporation www.schroff.com ABAQUS for CATIA V5,
More informationMoment-rotation Behavior of Shallow Foundations with Fixed Vertical Load Using PLAXIS 3D
6 th International Conference on Earthquake Geotechnical Engineering 1-4 November 2015 Christchurch, New Zealand Moment-rotation Behavior of Shallow Foundations with Fixed Vertical Load Using PLAXIS 3D
More informationTUTORIAL 7: Stress Concentrations and Elastic-Plastic (Yielding) Material Behavior Initial Project Space Setup Static Structural ANSYS ZX Plane
TUTORIAL 7: Stress Concentrations and Elastic-Plastic (Yielding) Material Behavior In this tutorial you will learn how to recognize and deal with a common modeling issues involving stress concentrations
More informationVisit the following websites to learn more about this book:
Visit the following websites to learn more about this book: 6 Introduction to Finite Element Simulation Historically, finite element modeling tools were only capable of solving the simplest engineering
More informationIJMH - International Journal of Management and Humanities ISSN:
EXPERIMENTAL STRESS ANALYSIS SPUR GEAR USING ANSYS SOFTWARE T.VADIVELU 1 (Department of Mechanical Engineering, JNTU KAKINADA, Kodad, India, vadimay28@gmail.com) Abstract Spur Gear is one of the most important
More informationFinite 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 informationDeep Beam With Web Opening
Deep Beam With Web Opening Name: Path: Keywords: DeepBeamWithWebOpening/deepbeam /Examples//DeepBeamWithWebOpening/deepbeam analys: linear static. constr: suppor. elemen: cq16m ct12m pstres. load: force
More informationModule: 2 Finite Element Formulation Techniques Lecture 3: Finite Element Method: Displacement Approach
11 Module: 2 Finite Element Formulation Techniques Lecture 3: Finite Element Method: Displacement Approach 2.3.1 Choice of Displacement Function Displacement function is the beginning point for the structural
More information