ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis

Size: px
Start display at page:

Download "ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis"

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 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 information

file://c:\documents and Settings\sala\Configuración local\temp\~hha54f.htm

file://c:\documents and Settings\sala\Configuración local\temp\~hha54f.htm Página 1 de 26 Tutorials Chapter 2. Structural Tutorial 2.1. Static Analysis of a Corner Bracket 2.1.1. Problem Specification Applicable ANSYS Products: Level of Difficulty: Interactive Time Required:

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

Example Plate with a hole

Example Plate with a hole Course in ANSYS Example Plate with a hole A Objective: Determine the maximum stress in the x-direction for point A and display the deformation figure Tasks: Create a submodel to increase the accuracy of

More information

Two Dimensional Truss

Two Dimensional Truss Two Dimensional Truss Introduction This tutorial was created using ANSYS 7.0 to solve a simple 2D Truss problem. This is the first of four introductory ANSYS tutorials. Problem Description Determine the

More information

NonLinear Materials AH-ALBERTA Web:

NonLinear Materials AH-ALBERTA Web: NonLinear Materials Introduction This tutorial was completed using ANSYS 7.0 The purpose of the tutorial is to describe how to include material nonlinearities in an ANSYS model. For instance, the case

More information

Bell Crank. Problem: Joseph Shigley and Charles Mischke. Mechanical Engineering Design 5th ed (New York: McGraw Hill, May 2002) page 87.

Bell 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 information

Module 1.2: Moment of a 1D Cantilever Beam

Module 1.2: Moment of a 1D Cantilever Beam Module 1.: Moment of a 1D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry Preprocessor 6 Element Type 6 Real Constants and Material Properties 7 Meshing 9 Loads 10 Solution

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

Structural static analysis - Analyzing 2D frame

Structural static analysis - Analyzing 2D frame Structural static analysis - Analyzing 2D frame In this tutorial we will analyze 2D frame (see Fig.1) consisting of 2D beams with respect to resistance to two different kinds of loads: (a) the downward

More information

ANSYS. Geometry. Material Properties. E=2.8E7 psi v=0.3. ansys.fem.ir Written By:Mehdi Heydarzadeh Page 1

ANSYS. 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 information

Course in ANSYS. Example0153. ANSYS Computational Mechanics, AAU, Esbjerg

Course in ANSYS. Example0153. ANSYS Computational Mechanics, AAU, Esbjerg Course in Example0153 Example Offshore structure F Objective: Display the deflection figure and von Mises stress distribution Tasks: Import geometry from IGES. Display the deflection figure? Display the

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

ANSYS Tutorials. Table of Contents. Grady Lemoine

ANSYS Tutorials. Table of Contents. Grady Lemoine ANSYS Tutorials Grady Lemoine Table of Contents Example 1: 2-D Static Stress Analysis in ANSYS...2 Example 2: 3-D Static Stress Analysis...5 Example 3: 2-D Frame With Multiple Materials and Element Types...10

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

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

Module 3: Buckling of 1D Simply Supported Beam

Module 3: Buckling of 1D Simply Supported Beam Module : Buckling of 1D Simply Supported Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Solution

More information

Structural static analysis - Analyzing 2D frame

Structural static analysis - Analyzing 2D frame Structural static analysis - Analyzing 2D frame In this tutorial we will analyze 2D frame (see Fig.1) consisting of 2D beams with respect to resistance to two different kinds of loads: (a) the downward

More information

Example Cantilever beam

Example Cantilever beam Course in ANSYS Example0300 Example Cantilever beam Objective: Compute the maximum deflection and locate point of maximum deflection Tasks: How should this be modelled? Compare results with results obtained

More information

5. Shell Reinforcement According To Eurocode 2

5. Shell Reinforcement According To Eurocode 2 5. Shell Reinforcement According To Eurocode Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 5 minutes Discipline: Concrete Shell Reinforcement

More information

Ansys Lab Frame Analysis

Ansys 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 information

Module 1.7: Point Loading of a 3D Cantilever Beam

Module 1.7: Point Loading of a 3D Cantilever Beam Module 1.7: Point Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 6 Element Type 6 Material Properties 7 Meshing 8 Loads 9 Solution 15 General

More information

ANSYS Mechanical APDL Tutorials

ANSYS 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 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

Release 10. Kent L. Lawrence. Mechanical and Aerospace Engineering University of Texas at Arlington SDC PUBLICATIONS

Release 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 information

ANSYS Tutorial Release 11.0

ANSYS 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 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

Latch Spring. Problem:

Latch 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 information

3. Check by Eurocode 3 a Steel Truss

3. 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 information

Analysis Steps 1. Start Abaqus and choose to create a new model database

Analysis 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 information

Statically Indeterminate Beam

Statically 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 information

Modelling and Analysis Lab (FEA)

Modelling 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 information

Structural modal analysis - 2D frame

Structural modal analysis - 2D frame Structural modal analysis - 2D frame Determine the first six vibration characteristics, namely natural frequencies and mode shapes, of a structure depicted in Fig. 1, when Young s modulus= 27e9Pa, Poisson

More information

6. Results Combination in Hexagonal Shell

6. Results Combination in Hexagonal Shell 6. Results Combination in Hexagonal Shell Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 0 minutes Discipline: Load combinations results Analysis

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

Lecture # 5 Modal or Dynamic Analysis of an Airplane Wing

Lecture # 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 information

TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS.

TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. Ex_1_2D Plate.doc 1 TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. 1. INTRODUCTION Two-dimensional problem of the theory of elasticity is a particular

More information

Melting Using Element Death

Melting 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 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

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

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

ANSYS EXERCISE ANSYS 5.6 Temperature Distribution in a Turbine Blade with Cooling Channels

ANSYS 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 information

Dhanalakshmi College Of Engineering

Dhanalakshmi 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 information

ME 442. Marc/Mentat-2011 Tutorial-1

ME 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 information

Course in ANSYS. Example0303. ANSYS Computational Mechanics, AAU, Esbjerg

Course in ANSYS. Example0303. ANSYS Computational Mechanics, AAU, Esbjerg Course in Example0303 Example Gear axle 3D Objective: Compute the maximum stress von Mise Tasks: How should this be modeled? Topics: Element type, Real constants, modeling, Plot results, output graphics,

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

Transient Thermal Conduction Example

Transient Thermal Conduction Example Transient Thermal Conduction Example Introduction This tutorial was created using ANSYS 7.0 to solve a simple transient conduction problem. Special thanks to Jesse Arnold for the analytical solution shown

More information

Essay 5 Tutorial for a Three-Dimensional Heat Conduction Problem Using ANSYS

Essay 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 information

Course in ANSYS. Example Truss 2D. Example0150

Course 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 information

Institute of Mechatronics and Information Systems

Institute of Mechatronics and Information Systems EXERCISE 4 Free vibrations of an electrical machine model Target Getting familiar with the fundamental issues of free vibrations analysis of a simplified model of an electrical machine, with the use of

More information

Course in ANSYS. Example0410. ANSYS Computational Mechanics, AAU, Esbjerg

Course in ANSYS. Example0410. ANSYS Computational Mechanics, AAU, Esbjerg Course in Example0410 Example Frame 2D Objective: Compute the harmonic response Tasks: Perform a modal analysis Display the mode shapes Perform a harmonic analysis Topics: Topics: Start of analysis, Element

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

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

Module 1.7W: Point Loading of a 3D Cantilever Beam

Module 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 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

Course in ANSYS. Example0505. ANSYS Computational Mechanics, AAU, Esbjerg

Course 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 information

CHAPTER 8 FINITE ELEMENT ANALYSIS

CHAPTER 8 FINITE ELEMENT ANALYSIS If you have any questions about this tutorial, feel free to contact Wenjin Tao (w.tao@mst.edu). CHAPTER 8 FINITE ELEMENT ANALYSIS Finite Element Analysis (FEA) is a practical application of the Finite

More information

Chapter 3. Thermal Tutorial

Chapter 3. Thermal Tutorial Chapter 3. Thermal Tutorial Tutorials> Chapter 3. Thermal Tutorial Solidification of a Casting Problem Specification Problem Description Prepare for a Thermal Analysis Input Geometry Define Materials Generate

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

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

Coupled Structural/Thermal Analysis

Coupled 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 information

Exercise 1: Axle Structural Static Analysis

Exercise 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 information

Generative Part Structural Analysis Fundamentals

Generative Part Structural Analysis Fundamentals CATIA V5 Training Foils Generative Part Structural Analysis Fundamentals Version 5 Release 19 September 2008 EDU_CAT_EN_GPF_FI_V5R19 About this course Objectives of the course Upon completion of this course

More information

COMPUTER AIDED ENGINEERING. Part-1

COMPUTER AIDED ENGINEERING. Part-1 COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.

More information

Course in ANSYS. Example0500. ANSYS Computational Mechanics, AAU, Esbjerg

Course 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 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

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 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

Outline. 3 Linear Analysis 3.1 Analysis commands 3.2 Results. Box Girder Bridge 2/28

Outline. 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 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

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

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

Modeling a Shell to a Solid Element Transition

Modeling 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 information

IJMH - International Journal of Management and Humanities ISSN:

IJMH - 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 information

16 SW Simulation design resources

16 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 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

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

Finite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench

Finite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench Finite Element Analysis using ANSYS Mechanical APDL & ANSYS Workbench Course Curriculum (Duration: 120 Hrs.) Section I: ANSYS Mechanical APDL Chapter 1: Before you start using ANSYS a. Introduction to

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

Figure E3-1 A plane struss structure under applied loading. Start MARC Designer. From the main menu, select STATIC STRESS ANALYSIS.

Figure 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 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

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

Course in ANSYS. Example0154. ANSYS Computational Mechanics, AAU, Esbjerg

Course 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 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

LAB MANUAL. Dharmapuri ME6711-SIMULATION AND ANALYSIS. Regulation : Branch : B.E. Mechanical Engineering

LAB 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 information

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

INTRODUCTION TO THE SYSTEM

INTRODUCTION 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 information

ABAQUS for CATIA V5 Tutorials

ABAQUS 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 information

Introduction to MSC.Patran

Introduction 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 information

FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS

FINITE 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 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

Assignment in The Finite Element Method, 2017

Assignment 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 information

Statically Indeterminate Beam

Statically 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 information

General modeling guidelines

General 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 information

Quick Start Guide to midas NFX

Quick 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 information

Course in ANSYS. Example0601. ANSYS Computational Mechanics, AAU, Esbjerg

Course 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 information

FINITE ELEMENT ANALYSIS LABORATORY MANUAL ANSYS. Course Instructor: Dr. R.Ganesan

FINITE 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 information

Institute of Mechatronics and Information Systems

Institute of Mechatronics and Information Systems EXERCISE 2 Free vibrations of a beam arget Getting familiar with the fundamental issues of free vibrations analysis of elastic medium, with the use of a finite element computation system ANSYS. Program

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

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