ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis
|
|
- Peter Campbell
- 6 years ago
- Views:
Transcription
1 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 for performing a simple analysis. This problem is a simple 2 dimensional static structural problem of a simple bracket as shown in the figure. This bracket is made of a 20 mm thick steel plate. The material properties of steel are given below: Young s modulus or Elastic Modulus, E = 200x10 9 Pascals Poisson s ratio, γ = 0.3 Density, ρ = 7860 kg/m 3 R10(TYP) PLATE THICKNESS: 20 mm ALL DIM IN mm 60 P=1000N R30 R20(TYP) 80 Loading and Boundary conditions: The plate is to be welded at the two smaller weld holes and a point load of 1000 N has to be applied along the y-axis as shown. The welded holes restrain the model in both x and y directions. 2. Approach and Assumptions: We assume this problem to be a 2 dimensional problem as the applied loads and the boundary conditions are in the x-y plane only. The thickness can be taken into account into the calculations in ANSYS without actually modeling in 3D. The approach is to model the bracket as a 2D solid model and generate the elements and mesh automatically. We can also create the nodes and elements separately. But such an approach would be a waste of time for a simple model as given in the example.
2 3. Summary of Steps: a) Preprocessing: - Create the solid model. - Choose the element type. - Assign real constants for the chosen element type - Assign material properties. - Mesh the model. b) Solution: - Apply the displacement boundary conditions - Apply the loads - Solve the model c) Post processing: - Read the results. - Plot the deformed shape. Compare with the undeformed shape. - Plot the von Mises stress. - Animate the stress output and study the trend - List the reaction solution - Exit ANSYS Outline of Hand-out Conventions: Before entering ANSYS 5.6, here is an outline of the layout of the tutorial handout. The handout starts from, How to enter ANSYS 5.6? to How to end session? However, the user may find some problems due to the version of ANSYS or some lack of continuity in the handout or due to a different operating system. The user may contact the instructor for clarifications. This tutorial is designed for use on ANSYS 5.6 operating on Windows 95/97/2000 or Windows NT. Also the tutorials follows the GUI mode (Graphic User Interface). Whenever the handout has commands in ITALICS, it means that the user should follow the menu options as directed. There would also be a description of the operation performed to help the user to understand what he is doing. The handout will also provide with pictures, tables and menus as it appears on the ANSYS window for more clarity. The Analysis procedure described in the handout may not be the only procedure to do the analysis. Neither is it the easiest procedure. But it has been designed such that the user gets exposed to as much options as possible. 5. Starting ANSYS 5.6: Start -> Programs -> Engineering Programs -> ANSYS 5.6 -> Interactive In the opened window, change the working directory to C:\temp Run You have now entered the ANSYS workspace. You can find that the main menu of ANSYS is open. If not, go to MenuCtrls -> Main Menu
3 6. File Operations: 6.1 Title of Analysis: In the Utility menu bar (the menu bar on the top of the screen), go to File -> Change Title. You can give a title name of your choice. Say, Static Analysis of a Bracket. 6.2 Analysis File Name: It is a good practice to give a file name even before you start the analysis. File -> Save As One more word of caution. ANSYS does not save the analysis into your file name when you give File -> Save. Instead it saves it into the default filename file.db. So every time to save a file, we have to say File -> Save As and overwrite the existing file. 7. Creating the Model: This is the first step of preprocessing. Preprocessing is the ANSYS analysis phase where you provide data regarding the geometry, element type, material properties and meshing. It would be referred in ANSYS as PREP7. The model can be created in many different ways. One of the easiest ways is to use the Rectangle and Circle Primitives Primitives are simple predefined geometric shapes ANSYS provides - as effectively as possible. So the geometry is to be viewed as an assemblage of circles and rectangles. a) Define the Rectangle: The first step is to create a base rectangle to which circles and other rectangles are to be added upon or subtracted from. Let us consider the lower left corner of the bracket as the origin. Main Menu > Preprocessor -> (-Modeling-) Create -> (-Areas-) Rectangle -> By 2 Corners
4 CAUTION: It is the responsibility of the user to ensure that the consistency of units be maintained throughout the analysis. It is best to first solve a simple problem as given in the assignment for which the analytical results are available. Close the Rectangle Menu after creating it. b) Create the Circle: Main Menu > Preprocessor -> (-Modeling-) Create -> (-Areas-) Circle -> Solid Circle The area plot shows both rectangle and circle, which are areas, in the same color. To more clearly distinguish between areas, turn on area numbers and colors. The "Plot Numbering Controls" dialog box on the Utility Menu controls how items are displayed in the Graphics Window. By default, a "replot" is automatically performed upon execution of the dialog box. The replot operation will repeat the last plotting operation that occurred (in this case, an area plot). Utility Menu -> PlotCtrls -> Numbering -> Area numbering ON c) Adding the Circle and Rectangle: Main Menu > Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Add -> Areas The Select window opens. Select both the areas and press OK. Now you can see that the areas are merged into a single area and the area number and color is also single. d) Creating the R30 bigger hole: As in the previous case, we have to first draw the circle and then perform the Boolean operation to subtract that area from the original area Main Menu > Preprocessor -> (-Modeling-) Create -> (-Areas-) Circle -> Solid Circle Main menu > Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Subtract -> Areas
5 CIRCLE CREATION MENU BOOLEAN (Subtraction) MENU During the Boolean Subtraction - Pick the area from which subtraction is going to take place(the bigger area, A3), PRESS OK. Then Pick area which is being subtracted (smaller area, A1), PRESS OK. e) To create the Fillet: To create the Fillet, we have to first create the Line Fillet. Then an area is created by the enclosure formed by the line fillet and then performing the Boolean Subtraction to subtract the fillet area from the main area. It is better to operate with lines when we create a line fillet. Utility Menu -> Plot -> Lines Main Menu -> Preprocessor ->(-Modeling-) Create -> (-Lines-)Line Fillet As shown in the adjoining figure, the lines that are to be filleted are selected and the fillet radius is given as 20. This creates the line fillet over the already existing area. So we have to create an area by the lines encompassing this fillet and subtract it from the bracket area.
6 Main Menu > Preprocessor -> (-Modeling-) Create -> (-Areas-) Arbitrary -> By Lines In the select window, select the 3 lines that make the area of the first fillet and click apply. Then select the area which form the second fillet and select OK Main menu > Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Subtract -> Areas Now pick the bracket area (Base area from which subtraction is done) and press OK in the Pick Window. Then pick the Fillet areas (Areas to be subtracted) and press OK. f) To create the Weld Holes: Similar to the R 30 hole which we created in step (b), we can create the two weld holes with the following parameters. Parameter Weld Hole 1 Weld Hole 2 WP X WP Y Radius Main Menu > Preprocessor -> (-Modeling-) Create -> (-Areas-) Circle -> Solid Circle Main menu > Preprocessor -> (-Modeling-) Operate -> (-Boolean-) Subtract -> Areas The completed geometry would look like the figure below SAVE AS.. Ur Filename.db
7 8. Element Type, Real Constants and Material Properties: a) Element Types - Indicates the element types used in the problem; over 100 element types are available in ANSYS. You choose an element type which characterizes, among other things, the degree-of-freedom set (displacements and/or rotations, temperatures, etc.) the characteristic shape of the element (line, quadrilateral, brick, etc.), whether the element lies in 2-D space or 3-D space, the response of your system, and the accuracy level you're interested in. For this analysis, we can use a 8 noded structural solid element called PLANE82. Since our system is of relatively simple geometry and loading, PLANE82 is sufficient. Results can be made accurate by having a very fine mesh. Main Menu -> Preprocessor -> Element type -> Add/Edit/Delete -> Structural Family of Elements -> Solid -> Quad 8 node 82 -> OK To account for the thickness of the bracket, the element options is selected to include calculation of stress including the thickness of the bracket. Defined Element type Window -> Options -> (Pull down Menu) Element Behavior K3 -> Plane strs w/thk. ELEMENT DEFINITION ELEMENT OPTION DEFINITION b) Real Constants: Real constants provide additional geometry information for element types whose geometry is not fully defined by its node locations. Typical real constants include shell thickness for shell elements and cross-sectional properties for beam elements. All properties required as input for a particular element type are entered as one set of real constants. Main Menu -> Preprocessing -> Real constants -> Add ->Real Constant Set Number -> THK 20
8 c) Material Properties: Physical properties of a material such as modulus of elasticity or density that are independent of geometry. Although they are not necessarily tied to the element type, the material properties required to solve the element matrices are listed for each element type for your convenience. Depending on the application, material properties may be linear, nonlinear, and/or anisotropic. As with element types and real constants, you may have multiple material property sets (to correspond with multiple materials) within one analysis. Each set is given a reference number. Main Menu -> Preprocessing -> MaterialProps -> (-Constant-) Isotropic Give the material a number label and press OK. Input the material properties in the Material property window. ANSYS provides us with a library of materials also. For accessing this library, we have to find the path name under the ANSYS directory for MATLIB directory. Main Menu -> Preprocessing -> MaterialProps -> Material Library -> Library path The Library path typically would be something like this, c:\ansys56\matlib Once you have entered the library, you can select from the list of materials available in ANSYS. Main Menu -> Preprocessing -> MaterialProps -> Material Library -> Import Library
9 9. The Meshing Process: Having defined the material properties, element type and the real constants, we can go ahead and mesh the model. One nice feature available in ANSYS is that we can generate the mesh automatically without breaking our heads to calculate the optimum mesh size. Depending on the degree of refinement required, we can choose either a course or a fine mesh size. Depending on the generated mesh, we can even refine it further. Main menu -> Preprocessor -> (-Meshing-) Size Cntrls -> (-Manual Size-) (-Global-)Size In the Size field, enter the number 5. This means that the element is to have a nominal size of 5x5 mm 2. Press OK Main menu -> Preprocessor -> (-Meshing-) Mesh -> (-Areas-) Free Pick the area to be meshed and press OK. You should be getting a mesh close to the one shown below. SAVE AS.. filename.db 10. Loads and Constraints: Now we have started the SOLUTION phase of the analysis. ANSYS analysis phase where you define analysis type and options, apply loads and load options, and initiate the finite element solution. A new, static analysis is the default. a) Application of Displacement Constraints: As described in the problem description, the 2 smaller holes are to be welded from the inside. This means that the degrees of freedom (dofs) are zero in the x and y directions i.e. no displacements in the x and y directions. Main Menu -> Solution -> (-Loads-) Apply ->(-Structural-) Displacement -> On Lines Pick the lines that comprise the weld holes and press OK.
10 Pick All DOF under Lab2 -> Enter 0 for Value. This simulates the effect of a rigidly welded hole in actual practice. b) Application of a Point Load: As specified in the problem, a vertical load of 1000 N has to be applied on the larger hole at the bottom quadrant point. Main Menu -> Solution ->(-Loads-) Apply -> Force/Moment -> On Keypoints Pick the Keypoint in the lower quadrant and press OK. In the Load Window, Choose the direction of force to be Fy. The Apply as field is to be set at the default value of Constant Value In the Force/Moment Value, Input force value as 1000 as the force is a downward (-ve y) acting force. 11. SOLUTION: Now we have finished modeling, meshing and defining the loads of the model. Now we have to solve the model and get the results. The default setting for solution control holds good for such a model. We have to modify the solution controls for different types of analysis as the case demands. Main Menu -> Solution -> (-Solve-) Current LS. The above command indicates that we are solving for the current load step. Once you click on the OK button, a dialog box that shows the different input parameters appears. We need to review the parameters and when we find it to be satisfactory, we can start the solution by pressing OK after closing the dialog box. If the model is good, a dialog box appears to say that the solution is done. The solutions are stored in the results file file.rst as this is a structural analysis. If it had been a thermal analysis, the results file is file.rth. SAVE_AS jobname.db
11 12. POST PROCESSING: The model has been solved and the user now has to invoke the POSTPROCESSING to view the results in a user-friendly manner. The postprocessor processes the results of the FEA, which is a huge 2n x 1 matrix of the displacements in the x and y directions, into user friendly plots. Also the post processor calculates other derived quantities like Stress, Strain, Strain energy etc. for the user to peruse. Main Menu -> Postprocessing -> (-Read Results-) Last Set The above command reads the final iteration result of the analysis. a) To plot the deformed shape: Main Menu -> Postprocessing -> Plot Results -> Deformed Shape Now we select Def + Undefrmed press OK. We should get an output that should resemble something like the figure given below.
12 b) To plot the von Mises Stress field: Main Menu -> Postprocessing -> Plot Results ->(-Contour Plot-) -> Nodal Solution In the plot results window, click on the Stress field and on the right hand box, scroll down till we find von Mises SEQV. The dialogue box would look like this. Press OK. The results would look something like the plot given below.
13 13. Modifying the loads and reviewing the results: This section is an extension of the previous model for the student to gain more insight into the analysis powers of ANSYS. The user has to go back to the solution and delete the point load and apply other types of loads. a) Try out with a pressure of N/m 2 acting on the lower quadrant of the bigger hole. b) Include into the above model the effect of self-weight by including the gravitational loads Gravitational loads are listed in Main Menu -> Solution ->(-Loads-) Apply ->Gravity c) Compare the results of the above two models. d) While solving the model with the gravity observe the solution status window before solving. The solution status window is the one given below. 14. Quitting ANSYS 5.6: Utility Menu -> File -> Exit ->. On the window, pick on Quit, No Save References: ANSYS Structural Analysis Command Guide
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
More informationfile://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:
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 informationExample 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
More informationTwo 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
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 informationBell Crank. Problem: Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed (New York: McGraw Hill, May 2002) page 87.
Problem: A cast-iron bell-crank lever, depicted in the figure below is acted upon by forces F 1 of 250 lb and F 2 of 333 lb. The section A-A at the central pivot has a curved inner surface with a radius
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 informationECE421: 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 informationStructural 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
More informationANSYS. Geometry. Material Properties. E=2.8E7 psi v=0.3. ansys.fem.ir Written By:Mehdi Heydarzadeh Page 1
Attention: This tutorial is outdated, you will be redirected automatically to the new site. If you are not redirected, click this link to the confluence site. Problem Specification Geometry Material Properties
More informationCourse 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
More informationNonLinear 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 informationANSYS 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
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 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 informationModule 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
More informationStructural 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
More informationExample 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
More information5. 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
More informationAnsys Lab Frame Analysis
Ansys Lab Frame Analysis Analyze the highway overpass frame shown in Figure. The main horizontal beam is W24x162 (area = 47.7 in 2, moment of inertia = 5170 in 4, height = 25 in). The inclined members
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 informationANSYS Mechanical APDL Tutorials
ANSYS Mechanical APDL Tutorials ANSYS, Inc. Southpointe 275 Technology Drive Canonsburg, PA 15317 ansysinfo@ansys.com http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494 Release 13.0 November 2010 ANSYS,
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 informationRelease 10. Kent L. Lawrence. Mechanical and Aerospace Engineering University of Texas at Arlington SDC PUBLICATIONS
ANSYS Release 10 Tutorial Kent L. Lawrence Mechanical and Aerospace Engineering University of Texas at Arlington SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com
More informationANSYS Tutorial Release 11.0
ANSYS Tutorial Release 11.0 Structural & Thermal Analysis Using the ANSYS Release 11.0 Environment Kent L. Lawrence Mechanical and Aerospace Engineering University of Texas at Arlington SDC PUBLICATIONS
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 informationLatch Spring. Problem:
Problem: Shown in the figure is a 12-gauge (0.1094 in) by 3/4 in latching spring which supports a load of F = 3 lb. The inside radius of the bend is 1/8 in. Estimate the stresses at the inner and outer
More information3. Check by Eurocode 3 a Steel Truss
TF 3. Check by Eurocode 3 a Steel Truss Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 40 minutes Discipline: Structural Steel Analysis Type:
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 informationStatically Indeterminate Beam
Problem: Using Castigliano's Theorem, determine the deflection at point A. Neglect the weight of the beam. W 1 N/m B 5 cm H 1 cm 1.35 m Overview Anticipated time to complete this tutorial: 45 minutes Tutorial
More informationModelling and Analysis Lab (FEA)
Channabasaveshwara Institute of Technology (Affiliated to VTU, Belagavi & Approved by AICTE, New Delhi) (NAAC Accredited & ISO 9001:2015 Certified Institution) NH 206 (B.H. Road), Gubbi, Tumakuru 572 216.
More informationStructural 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
More information6. 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
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 informationLecture # 5 Modal or Dynamic Analysis of an Airplane Wing
Lecture # 5 Modal or Dynamic Analysis of an Airplane Wing Problem Description This is a simple modal analysis of a wing of a model airplane. The wing is of uniform configuration along its length and its
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 informationMelting Using Element Death
Melting Using Element Death Introduction This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to outline the steps required to use element death to model melting of a material. Element
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 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 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 informationANSYS EXERCISE ANSYS 5.6 Temperature Distribution in a Turbine Blade with Cooling Channels
I. ANSYS EXERCISE ANSYS 5.6 Temperature Distribution in a Turbine Blade with Cooling Channels Copyright 2001-2005, John R. Baker John R. Baker; phone: 270-534-3114; email: jbaker@engr.uky.edu This exercise
More informationDhanalakshmi College Of Engineering
Dhanalakshmi College Of Engineering Manimangalam, Tambaram, Chennai 601 301 DEPARTMENT OF MECHANICAL ENGINEERING ME 6711 SIMULATION AND ANALYSIS LABORATORY VII SEMESTER - R 2013 LABORATORY MANUAL Name
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 informationCourse 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,
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 informationTransient 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
More informationEssay 5 Tutorial for a Three-Dimensional Heat Conduction Problem Using ANSYS
Essay 5 Tutorial for a Three-Dimensional Heat Conduction Problem Using ANSYS 5.1 Introduction The problem selected to illustrate the use of ANSYS software for a three-dimensional steadystate heat conduction
More informationCourse in ANSYS. Example Truss 2D. Example0150
Course in ANSYS Example0150 Example Truss 2D Objective: Compute the maximum deflection Tasks: Display the deflection figure? Topics: Topics: Start of analysis, Element type, Real constants, Material, modeling,
More informationInstitute 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
More informationCourse 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
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 informationCreating 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 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 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 informationCourse in ANSYS. Example0505. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0505 Example Plate Objective: Compute the buckling load Tasks: How should this be modelled? Compare results with results obtained from norm calculations? Topics: Element type, Real constants,
More informationCHAPTER 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
More informationChapter 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
More informationFinite 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 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 informationCoupled Structural/Thermal Analysis
Coupled Structural/Thermal Analysis Introduction This tutorial was completed using ANSYS 7.0 The purpose of this tutorial is to outline a simple coupled thermal/structural analysis. A steel link, with
More informationExercise 1: Axle Structural Static Analysis
Exercise 1: Axle Structural Static Analysis The purpose of this exercise is to cover the basic functionality of the Mechanical Toolbar (MTB) in the context of performing an actual analysis. Details of
More informationGenerative 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
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 informationCourse in ANSYS. Example0500. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0500 Example Column beam Objective: Compute the critical buckling load and display the mode shape Tasks: Create a table and compare results with results obtained from buckling theory?
More informationCE366/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 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 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 informationOutline. 3 Linear Analysis 3.1 Analysis commands 3.2 Results. Box Girder Bridge 2/28
ANALYS: linear static. CONSTR: suppor. ELEMEN: bar hx24l reinfo solid tp18l. LOAD: elemen face force prestr reinfo weight. MATERI: elasti isotro. OPTION: direct. POST: binary ndiana. PRE: dianai. RESULT:
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 informationCHAPTER 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 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 informationModeling a Shell to a Solid Element Transition
LESSON 9 Modeling a Shell to a Solid Element Transition Objectives: Use MPCs to replicate a Solid with a Surface. Compare stress results of the Solid and Surface 9-1 9-2 LESSON 9 Modeling a Shell to a
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 information16 SW Simulation design resources
16 SW Simulation design resources 16.1 Introduction This is simply a restatement of the SW Simulation online design scenarios tutorial with a little more visual detail supplied on the various menu picks
More informationAbaqus 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 informationRevised 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 informationFinite 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
More information1.992, 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 informationFigure E3-1 A plane struss structure under applied loading. Start MARC Designer. From the main menu, select STATIC STRESS ANALYSIS.
Example 3 Static Stress Analysis on a Plane Truss Structure Problem Statement: In this exercise, you will use MARC Designer software to carry out a static stress analysis on a simple plane truss structure,
More informationPro 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 informationAbaqus 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 informationCourse in ANSYS. Example0154. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0154 Example Frame 2D E = 210000N/mm 2 n = 0.3 L= 1000mm H = 1000mm a = 20mm b = 50mm c = 400mm F = 10000N I = 208333N/mm 4 Example0154 2 Example Frame 2D Objective: Compute the maximum
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 informationLAB MANUAL. Dharmapuri ME6711-SIMULATION AND ANALYSIS. Regulation : Branch : B.E. Mechanical Engineering
Dharmapuri 636 703 LAB MANUAL Regulation : Branch : 2013 B.E. Mechanical Engineering Year & Semester : IV Year / VII Semester ME6711-SIMULATION AND ANALYSIS Varuvan Vadivelan Institute of Technology, Dharmapuri
More informationME 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 informationINTRODUCTION TO THE SYSTEM
INTRODUCTION TO THE SYSTEM 1 INTRODUCTION TO THE SYSTEM 1. Introduction The ANSYS computer program is a large-scale multi-purpose finite element program, which may be used for solving several classes of
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 informationIntroduction to MSC.Patran
Exercise 1 Introduction to MSC.Patran Objectives: Create geometry for a Beam. Add Loads and Boundary Conditions. Review analysis results. MSC.Patran 301 Exercise Workbook - Release 9.0 1-1 1-2 MSC.Patran
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
Problem Description: FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Dimitri Soteropoulos Programs Utilized: Abaqus/CAE 6.11-2 This tutorial explains how to build
More informationFinite 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 informationAssignment in The Finite Element Method, 2017
Assignment in The Finite Element Method, 2017 Division of Solid Mechanics The task is to write a finite element program and then use the program to analyse aspects of a surface mounted resistor. The problem
More informationStatically Indeterminate Beam
Problem: A rectangular aluminum bar.5 inches thick and 2 inches wide is welded to fixed supports at the ends, and the bar supports a load W=800 lb, acting through the pin as shown. Find the reactions at
More informationGeneral modeling guidelines
General modeling guidelines Some quotes from industry FEA experts: Finite element analysis is a very powerful tool with which to design products of superior quality. Like all tools, it can be used properly,
More informationQuick Start Guide to midas NFX
Quick Start Guide to midas NFX This guide is made for non-experienced FEA users. It provides basic knowledge needed to run midas NFX successfully and begin your analysis. Experienced FEA analysts can also
More informationCourse in ANSYS. Example0601. ANSYS Computational Mechanics, AAU, Esbjerg
Course in Example0601 Example Turbine Blade Example0601 2 Example Turbine Blade Objective: Solve for the temperature distribution within the 6mm thick turbine blade, with 2mm x 6mm rectangular cooling
More informationFINITE ELEMENT ANALYSIS LABORATORY MANUAL ANSYS. Course Instructor: Dr. R.Ganesan
FINITE ELEMENT ANALYSIS MECH 460 LABORATORY MANUAL ANSYS Course Instructor: Dr. R.Ganesan Prepared by A. Zabihollah Approved by Dr. R. Ganesan Winter 2007 Table of Contents 1. INTRODUCTION.3 1.1 Starting
More informationInstitute 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
More informationENGINEERING 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 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 information