Tutorial Week 10 Internal bone remodelling
|
|
- Julie Carroll
- 5 years ago
- Views:
Transcription
1 Introduction Tutorial Week 10 Internal bone remodelling This tutorial will introduce the necessary steps to simulate internal bone remodelling of an implanted femur using ANSYS. You will learn to: Setup and export mesh data from Workbench Generate an APDL input file for use with ANSYS Classic Call a pre-compiled Fortran subroutine during solution Step 1: Prepare geometries for the femur and implant The preparation of a realistic implanted femur geometry was detailed in week 4 s tutorial. This involved the removal of the head and neck of the segmented femur in ScanIP using the 3D editing tools. After completing the steps detailed in week 4 s tutorial, you should end up with the following femur bone geometry. Export this geometry from ScanIP as an IGS file. The femoral component of the hip implant is available for download on the course website (FemoralImplant.IGS), under the tutorial content for week 4, shown below.
2 Once you have both IGS geometries, they can be imported into Workbench. While it is possible to import geometries directly into ANSYS Classic, the CAD interfaces in Workbench are significantly more modern and work much better with external geometry files. Start a new Mechanical Model module in the Workbench project window. Double-click on geometry to open Design Modeler. Import both the femur and implant geometries. They should look something like this: The process of aligning these two geometries is provided in the week 4 tutorial. This involves a simple body translation to move the implant into the correct position as shown. Once correctly aligned, a cavity for the implant in the femur is required. Use the Boolean subtraction function provided in Design Modeler (Create > Boolean) to
3 create this cavity. Remember to select the femur as the target body and the implant as the tool body, and ensure Preserve tool bodies is enabled (Yes). Pay attention At this point, the instructions deviate from week 4 s tutorial. For this model, we are going to assume that the bone and implant are glued together. We could allow Workbench to apply the default bonded condition to the contact surfaces between these two geometries, but the simplest way to define this relationship is to form a single part. Do this by selecting both geometries in the tree outline, right-clicking and choosing Form New Part. For the mesh-savvy amongst you, forming a new part enforces a contiguous mesh between the implant and the bone. This means that the implant and bone will share the same nodes along their interface, effectively gluing the two bodies together, and negating the need for special contact conditions. The result will be a single part containing two individual bodies. Don t worry, separate material properties may still be assigned to these two bodies. Close the Design Modeler window, and it s probably a good idea to save your project file at this point. Step 2: Generating the mesh in Workbench Now the material properties can be set up in the Mechanical Model module. Open Engineering Data and make two isotropic elastic materials: Bone and Implant. It doesn t matter what Young s modulus and Poisson s ratio you specify in this section; they will just act as placeholders for the bone and implant mesh objects. A Young s modulus of 1 for the bone and Young s modulus of 2 for the implant will suffice. Close Engineering Data and open the Model component. This will launch the Mechanical application window. First, assign the bone and implant materials to their respective bodies. The next thing to do is generate a mesh for the model. For this
4 tutorial, it s sufficient to just keep most of the default mesh settings. However, you should keep element mid-side nodes to generate quadratic (second-order) elements. Do this in the Advanced section of Mesh details, as shown below. Although we should technically do a mesh convergence study to verify the accuracy of our finite element model, we re going to skip this for the sake of brevity. The last thing we need to do in the Mechanical application is to define a named selection for face on the neck of the femoral implant. Select the face and add it as a named selection as below. This will make it easier to apply forces using APDL.
5 Step 3: Using FE Modeler to export the mesh Once the mesh and named selection have been generated, close the Mechanical application window. Insert an Finite Element Modeler module into the Workbench project window, and link the model component of the Mechanical Model module to it. The FE Modeler module enables the export of mesh objects created in Workbench to a variety of formats, including to ANSYS Classic by creating an APDL input file. It will also translate the materials specified in Engineering Data and the Named Selections defined in the Mechanical application to their APDL analogues. Before opening FE Modeler, ensure that the unit used for the model are in metres, not millimetres. You can do this by checking the Properties of the Assembly Mesh in the Outline pane. If you don t see Outline and Properties panes, go to View > Outline and View > Properties in the project window. Open FE Modeler by double-clicking the Model component. Ensure that the Target System is Mechanical APDL. You can check out the features of your mesh in the outline tree. If all the instructions have been followed correctly, all you need to do is click on Write Solver File. This writes all the mesh data to an APDL input file. You can preview the contents of this file under Generate Data. Name your input file A3_mesh.inp so it can be identified later.
6 Step 4: Editing the generated APDL input file After saving the APDL input file from FE Modeler, close and save your Workbench project file. The remainder of this project will take you through the steps needed to create a solvable APDL input file. APDL input files are just text files. You can open them in any text editor. The input file generated from FE Modeler contains the locations of all the nodes, and the definitions of all the elements from those nodes, and is therefore quite large for a text file. Use Notepad++, which is available on the PCLAB computers, to open this input file. Your input file will probably start off like this: /PREP7 SHPP,OFF /NOPR COORDINATE SYSTEMS MATERIAL PROPERTIES /com, Materials <SECTION=MATERIALS> Origin Material Property ID - 23 MP,EX,1,1, Pa MP,NUXY,1,0.3, Origin Material Property ID - 25 MP,EX,2,2, Pa MP,NUXY,2,0.3, PHYSICAL PROPERTIES ELEMENT TYPES /com, Element Types <SECTION=ELEMENTTYPES> et,1,mesh200 keyopt,1,1,9 Some of these commands will be explained later in this tutorial when you work with the template input file. The character denotes a comment, as does the /com command. Briefly, the above set of commands opens the pre-processing module (PREP7), sets up two materials (MP), with Young s modulus (EX) and Poisson s ratio (NUXY), and then specifies a type of element to use (ET), which is called MESH200. The Young s modulus and Poisson s ratio of the materials you specified in Engineering Data previously should be reflected in the MP commands. All we want in this input file is the definition of the nodes, elements, and the named selection, which is called a component in APDL. So either delete, or comment out the above selection of commands. You should end up with the nodal listing (list of node numbers and their co-ordinates): nblock,3 (1i8,3e20.9e3) <nodes>
7 and the element listing (list of element numbers, the material number, element type, and the nodes that are used to construct them): eblock,19,solid,12307 (19i8) <elements> and the component listing (component from the Named Selection, and the associated node numbers): CMBLOCK,NECK,NODE, 37 (8i10) <nodes> Note that the CMBLOCK command, which is used to define the component, specifies 37 nodes. This is important later, when we apply forces on these nodes. Then go to the very end of the input file (Ctrl+End), and delete the following unnecessary commands. BOUNDARY CONDITIONS LOADS Solution Turn output back on /GOPR FINI /GOPR You can now save this input file. Step 5: Generating a solvable APDL input file Download the template APDL file from the course website, under the week 10 tutorial content, and open this in Notepad++. Most of the input file has been commented in-line, however some important commands will be detailed here. Full descriptions of each command and the associated options are detailed in ANSYS Help (under Mechanical APDL > Command Reference). To enable the set-up of model, /PREP7 command is issued to activate the preprocessing modules in ANSYS. After this, we can define the materials, mesh, and loads.
8 et,1,solid187 defines element type number 1 as a SOLID187, which is a 10- node tetrahedral element (10 nodes means it has mid-side nodes and therefore has quadratic shape functions). This matches the type of mesh we defined in Step 2. Next we need to define the material properties of the femur bone (material number 1). As the Young s modulus of the femur bone is going to change in response to a mechanical stimulus, TB,ELASTIC,1 is used to make a material table that can be used to define changing elastic material properties (i.e. Young s modulus and Poisson s ratio). In addition, we need a specify a user-defined field variable (UF01) that can be changed in this manner using a subroutine. In this example, UF01 is going to be the Young s modulus, so the relationship between UF01 and the Young s modulus in the material table is going to be perfectly linear (with a gradient of 1). We can make this happen by using the TBFIELD and TBDATA commands to define two points that will define a straight line. See the table below to see what this means. UF01 Young s modulus (Pa) This work-around allows us to directly change the Young s modulus of the bone by changing UF01 using a Fortran subroutine. Note that the Poisson s ratio will stay the same here. TB,STATE,,1 is another work-around in the APDL input that allows us to store custom data in the results. This defines a single state variable that we will use to store bone density, which will then be plotted after the model is solved. The implant is then given regular material properties using the MP command. You can change the numbers to give the implant a Young s modulus (EX) and Poisson s ratio (NUXY) of your own choosing. Next, it s time to import the mesh you defined in the A3_mesh.inp APDL file. You can insert it using: /INPUT,A3_MESH,inp. This type of command can be used to input any APDL code into the file without having to copy and paste it over. Following this are commands that give an initial value to the UF01 field variable that was defined earlier. The femur bone elements need this for the first time-step (before any bone remodelling has occurred). In this example, we ve assumed that the bone is completely homogeneous, and has a Young s modulus of approximately 10.5 GPa. To fix the base of the femur, the nodes on the bottom face of the femur need to be selected. The following commands select these nodes, set their displacements in the
9 X, Y, and Z directions to 0, and then re-select everything to prevent confusion with the following commands. NSEL,S,LOC,Z,-445.9e-3 D,ALL,UX,0 D,ALL,UY,0 D,ALL,UZ,0 ALLSEL Forces in the Z direction (FZ) can be applied onto the component/named selection that was defined from Workbench. Specify the name of the component (NECK) when issuing the F command. Forces can also be applied in the X (FX) and Y (FY) directions as well by issuing multiple commands. Note that the force is applied to each node, so we divide the total force by the number of nodes noted earlier in the component definition (37 nodes for the example given in Step 4). The final part of the APDL input file specifies the solution settings. antype,transient time,24 deltim,1 outres,all,all outres,svar,all solve finish save These commands specify a transient analysis type (ANTYPE), which will terminate at time = 24 (TIME), in increments of 1 (DELTIM), and export all the results for all the time-steps (OUTRES), including the state variable (SVAR) which will contain the bone density data. SOLVE executes the solution. SAVE creates a.db file that can be used to reopen the model in the ANSYS Classic GUI. You may add your own post-processing commands to save the bone density plots automatically after it finishes solving (see Appendix). Once you have completed creating the APDL input file, save it with a different filename (e.g. A3_solve.inp) Step 6: Solving using the pre-compiled USERFLD subroutine As described in the lecture, the APDL input is a high-level scripting language, which is interpreted line-by-line by the ANSYS program. In this tutorial, APDL input has been used to define the nodes and elements of the model, and set up the various boundary conditions and material properties. To simulate the internal remodelling in the femur bone, a USERFLD subroutine needs to be run at the end of every time-step to update the bone density, and therefore, the Young s modulus (which corresponded to the user-defined field, UF01 in the APDL file). These changes in Young s modulus affect the mechanical stimulus experienced by the femur bone in the next time-step. The subroutine is written in
10 Fortran, which is a lower-level programming language that needs to be compiled to an executable object before ANSYS can execute it. Luckily in this tutorial, we can use a pre-compiled subroutine, which saves a lot of trouble. The commented source code and pre-compiled objects necessary to solve the model are downloadable from the course website. Please download this and examine the source code (USERFLD.F) to identify the steps and relationships used to translate the mechanical stimulus to a change in bone density and Young s modulus. All the files should be placed in your working directory. It is ideal to make the working directory as a new folder on the Desktop if you are in the PCLAB. The most efficient way of running ANSYS is using the batch interface. From the Windows Start Menu, open cmd.exe. Use the cd command to navigate to your working directory. An example navigating to the folder assignment on the Desktop is provided below. cd C:\Users\your_unikey\Desktop\assignment Before we run our APDL input file (A3_solve.inp), ANSYS needs to know if there is a subroutine we would like to use, and where it is located. Let s assume you followed the instructions above and put all the pre-compiled files into the working directory (e.g. assignment ). Use the following commands to set a temporary ANSYS environmental variable, and check that it has been set properly. set ANS_USER_PATH=C:\Users\your_unikey\Desktop\assignment echo %ANS_USER_PATH% Finally, it is time to run ANSYS. C:\Program Files\ANSYS Inc\v161\ansys\bin\winx64\ansys161.exe b j A3 i A3_solve.inp o A3.out -b means batch mode -j specifies the job name (and the name of the files that get dumped in your working directory) -i specifies the name of the APDL input file -o specifies the name of an output file, from which you can monitor the status of your job and any errors or warnings that occur. On UNIX systems, there is a tool called tail, but on Windows, you can download a program called baretail.exe to watch the output file as new events get added to it. Once the job has completed successfully, you can open the generated.db file by double-clicking on it, which will open the ANSYS Classic GUI.
11 Step 7: Post-processing the results in ANSYS Classic Various toolbars and windows are highlighted: Yellow: Top Menu, contains options for most of the commands used in ANSYS Green: Scripting Bar, allowing for the entry of APDL commands Red: Main Menu, contains all the options and steps for modelling Blue: Graphics Window, the graphical display Orange: Viewing Tools, used for changing the view in the graphics window First, load the generated results for the first time-step. To do this use either: Main Menu > General Postproc > Read Results > First Set Enter the following APDL commands into the Scripting bar /POST1 set,,1 Since we are interested in the response of the femur bone, select just the bone elements. Select > Entities. Elements > By Attributes > Material num. Enter 1. esel,s,mat,,1 Plot some results, and use the viewing tools (orange) to move the model around. Main Menu > General Postproc > Plot Results > Nodal Solution > Stress > von Mises stress plnsol,s,eqv
12 Sometimes contour limits don t show enough of the distribution, so you can change them. PlotCtrls > Style > Contours > Uniform Contours > User specified /cont,,10,0,,1e6 /replot For the example /cont command, 10 is the number of contour levels, 0 is the minimum level, and 1e6 is the maximum level. Any results over the maximum contour level will show up as grey. If you find this disconcerting, you can change it to red. PlotCtrls > Style > Colors > Contour Colors > Color above contours /color,smax,red To plot bone density, which was stored as state variable, use the following command. plnsol,svar,1 You can use the same contour controls to show which parts of the bone remodel the most. Keep in mind that the first time-step shows no remodelling, as the bone starts off as a homogeneous 1800 kg/m 3. Bone density data is available for all remaining time-steps. A more advanced subroutine would include greyscale data from CT scans to create an initially inhomogeneous femur bone. Once you are done with the current time-step, move to the next one and so on. Main Menu > General Postproc > Read Results > Next Set Enter the following APDL commands into the Scripting bar set,,2 Appendix: Saving plots in ANSYS Classic/APDL You can use the ANSYS Classic GUI and/or APDL commands to export images of your model. With ANSYS Classic GUI, use the Viewing tools on the right to position the model ideally in the graphics window. Then redirect the plot to a file as follows: PlotCtrls > Redirect Plots > To PNG File. You can change the settings for background colour and resolution here, and upon Apply, it will write a.png image to your working directory (filename is based on the jobname). The fastest way to export a lot of plots is to use APDL commands. You can also use APDL to orient the model in your graphics window. For example, zoom extents (fit model to the window) and view along the x axis.
13 /AUTO,1 /VIEW,,1,0,0 /REPLOT Set zoom Set camera orientation (x,y,z) Refresh view Export some PNGs. /GFILE,1200 Set image res TIFF,COMP,1 Set PNG compression PNGR,ORIENT,HORIZONTAL Set orientation PNGR,COLOR,2 Set colour PNGR,TMOD,0 Set line strokes /SHOW,PNG,,0 Start PNG export PLNSOL,SVAR,1 First density plot *DO,i,2,24 Loop from 2 to 24 set,,i Change time-step /replot Refresh plot *ENDDO End loop /SHOW,CLOSE Stop PNG export Add this set of commands to some of the initial post-processing commands (/POST1 and the contour controls) and you can then put it in the solvable APDL input file. Alternatively, just save it in a text file, and read it in through the Classic GUI. File > Read Input From
Tutorial Week 4 Biomedical Modelling in Ansys Workbench (The Complete Guide with Anatomy and Implant)
Tutorial Week 4 Biomedical Modelling in Ansys Workbench (The Complete Guide with Anatomy and Implant) Step 1: Create the Anatomical Model in ScanIP Import the DICOM files for the Proximal Femur dataset
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 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 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 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 informationChapter 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 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 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 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 informationTutorial Week 7 Optimisation
Introduction Tutorial Week 7 Optimisation This tutorial will introduce the optimisation study technique using the Response Surface Method in Workbench. You will learn to: Import a SolidWorks geometry into
More informationSolving FSI Applications Using ANSYS Mechanical and ANSYS Fluent
Workshop Transient 1-way FSI Load Mapping using ACT Extension 15. 0 Release Solving FSI Applications Using ANSYS Mechanical and ANSYS Fluent 1 2014 ANSYS, Inc. Workshop Description: This example considers
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 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 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 informationTruss Bracket. Problem:
Problem: The truss structure shown above is mounted on the sides of buildings during construction for use as scaffolding for workers. A design team has created a new bracket design (shown below) to use
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 informationTorsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10
Torsional-lateral buckling large displacement analysis with a simple beam using Abaqus 6.10 This document contains an Abaqus tutorial for performing a buckling analysis using the finite element program
More informationANSYS Customization. Mechanical and Mechanical APDL. Eric Stamper. Presented by CAE Associates
ANSYS Customization Mechanical and Mechanical APDL Presented by Eric Stamper 2011 CAE Associates Introduction CAE Associates Inc. Engineering consulting firm since 1981. ANSYS consulting, custom software
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 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 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 5.6 Tutorials Lecture # 2 - Static Structural Analysis
R50 ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis Example 1 Static Analysis of a Bracket 1. Problem Description: The objective of the problem is to demonstrate the basic ANSYS procedures
More 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 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 informationThis tutorial will take you all the steps required to import files into ABAQUS from SolidWorks
ENGN 1750: Advanced Mechanics of Solids ABAQUS CAD INTERFACE TUTORIAL School of Engineering Brown University This tutorial will take you all the steps required to import files into ABAQUS from SolidWorks
More informationExercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0
Exercise 1 3-Point Bending Using the Static Structural Module of Contents Ansys Workbench 14.0 Learn how to...1 Given...2 Questions...2 Taking advantage of symmetries...2 A. Getting started...3 A.1 Choose
More informationModule 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 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 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 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 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 information[ ] u 1. ME309 Homework #2 $ % & u = 1 s 2 " # u 2. s,u. A,E constant along length. 4Etc
ME09 Homework # OBJECTIVES: Introduction to convergence issues and modeling approaches Postprocessing procedures Element selection Experience with shape functions and stiffness terms NOTES: Problems 1and
More informationEN1740 Computer Aided Visualization and Design Spring /26/2012 Brian C. P. Burke
EN1740 Computer Aided Visualization and Design Spring 2012 4/26/2012 Brian C. P. Burke Last time: More motion analysis with Pro/E Tonight: Introduction to external analysis products ABAQUS External Analysis
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 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 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 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 informationANSYS Tutorial Version 6
ANSYS Tutorial Version 6 Fracture Analysis Consultants, Inc www.fracanalysis.com Revised: November 2011 Table of Contents: 1.0 Introduction... 4 2.0 Tutorial 1: Crack Insertion and Growth in a Cube...
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 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 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 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 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 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 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 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 informationASME Fatigue DOCUMENTATION. ANSYS Mechanical Application. Extension version Compatible ANSYS version
ASME Fatigue ANSYS Mechanical Application DOCUMENTATION Extension version 180.1 Release date 06-Apr-17 Compatible ANSYS version 18.0 www.edrmedeso.com Table of Contents 1 INTRODUCTION... 3 2 PRODUCT RESTRICTIONS...
More informationThe Essence of Result Post- Processing
APPENDIX E The Essence of Result Post- Processing Objectives: Manually create the geometry for the tension coupon using the given dimensions then apply finite elements. Manually define material and element
More informationDMU Engineering Analysis Review
Page 1 DMU Engineering Analysis Review Preface Using This Guide Where to Find More Information Conventions What's New? Getting Started Inserting a CATAnalysis Document Using DMU Space Analysis From CATAnalysis
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 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 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 informationModule 1.3W Distributed Loading of a 1D Cantilever Beam
Module 1.3W Distributed Loading of a 1D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Workbench Analysis System 4 Engineering Data 5 Geometry 6 Model 11 Setup 13 Solution
More 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 informationDavid Wagner, Kaan Divringi, Can Ozcan Ozen Engineering
Internal Forces of the Femur: An Automated Procedure for Applying Boundary Conditions Obtained From Inverse Dynamic Analysis to Finite Element Simulations David Wagner, Kaan Divringi, Can Ozcan Ozen Engineering
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 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 informationDMU Engineering Analysis Review
DMU Engineering Analysis Review Overview Conventions What's New? Getting Started Entering DMU Engineering Analysis Review Workbench Generating an Image Visualizing Extrema Generating a Basic Analysis Report
More informationES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010
ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.
More informationSliding Split Tube Telescope
LESSON 15 Sliding Split Tube Telescope Objectives: Shell-to-shell contact -accounting for shell thickness. Creating boundary conditions and loads by way of rigid surfaces. Simulate large displacements,
More informationFinite Element Analysis Using 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 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 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 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 informationVOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL
VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL The following is a description of the model setups and input/output parameters for benchmarking analytical volcanic deformation models
More 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 informationIntroduction And Overview ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary
Introduction And Overview 2006 ANSYS, Inc. All rights reserved. 1 ANSYS, Inc. Proprietary The ANSYS Workbench represents more than a general purpose engineering tool. It provides a highly integrated engineering
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 informationInstallation Guide. Beginners guide to structural analysis
Installation Guide To install Abaqus, students at the School of Civil Engineering, Sohngaardsholmsvej 57, should log on to \\studserver, whereas the staff at the Department of Civil Engineering should
More informationLinear Bifurcation Buckling Analysis of Thin Plate
LESSON 13a Linear Bifurcation Buckling Analysis of Thin Plate Objectives: Construct a quarter model of a simply supported plate. Place an edge load on the plate. Run an Advanced FEA bifurcation buckling
More informationFEMORAL STEM SHAPE DESIGN OF ARTIFICIAL HIP JOINT USING A VOXEL BASED FINITE ELEMENT METHOD
FEMORAL STEM SHAPE DESIGN OF ARTIFICIAL HIP JOINT USING A VOXEL BASED FINITE ELEMENT METHOD Taiji ADACHI *, Hiromichi KUNIMOTO, Ken-ichi TSUBOTA #, Yoshihiro TOMITA + Graduate School of Science and Technology,
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Michael Schraiber, Dimitri Soteropoulos, Sanjay Nainani Programs Utilized: HyperMesh Desktop v2017.2, OptiStruct,
More informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More informationProblem description. It is desired to analyze the cracked body shown using a 3D finite element mesh: Top view. 50 radius. Material properties:
Problem description It is desired to analyze the cracked body shown using a 3D finite element mesh: Top view 30 50 radius 30 Material properties: 5 2 E = 2.07 10 N/mm = 0.29 All dimensions in mm Crack
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 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 informationVisit the following websites to learn more about this book:
Visit the following websites to learn more about this book: 6 Introduction to Finite Element Simulation Historically, finite element modeling tools were only capable of solving the simplest engineering
More 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 informationIntroduction To Finite Element Analysis
Creating a Part In this part of the tutorial we will introduce you to some basic modelling concepts. If you are already familiar with modelling in Pro Engineer you will find this section very easy. Before
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 informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
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 informationGetting Started. These tasks should take about 20 minutes to complete. Getting Started
Getting Started Getting Started This tutorial will guide you step-by-step through your first ELFINI and Generative Part Structural Analysis session, allowing you to get acquainted with the product. You
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 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 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 informationIntroduction: RS 3 Tutorial 1 Quick Start
Introduction: RS 3 Tutorial 1 Quick Start Welcome to RS 3. This tutorial introduces some basic features of RS 3. The model analyzes the effect of tank loading on an existing sloped underground tunnel.
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 informationTRINITAS. a Finite Element stand-alone tool for Conceptual design, Optimization and General finite element analysis. Introductional Manual
TRINITAS a Finite Element stand-alone tool for Conceptual design, Optimization and General finite element analysis Introductional Manual Bo Torstenfelt Contents 1 Introduction 1 2 Starting the Program
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 informationImpicit Delayed Norton Creep Implemented
Impicit Delayed Norton Creep Implemented Carlos Shultz PADT Inc. Abstract A custom implicit creep routine was developed. The routine was based upon Norton's creep equation using Hoop Stress with an additional
More informationStress analysis of toroidal shell
Stress analysis of toroidal shell Cristian PURDEL*, Marcel STERE** *Corresponding author Department of Aerospace Structures INCAS - National Institute for Aerospace Research Elie Carafoli Bdul Iuliu Maniu
More informationCase Study- Importing As-Molded Plastic Part Conditions into CAE tools
1 IEI Innova Engineering 1 Park Plaza Suite 980 Irvine, California 92614 Case Study- Importing As-Molded Plastic Part Conditions into CAE tools 2 CONTENTS CONTENTS... 2 EXECUTIVE SUMMARY... 3 APPROACH...
More informationChapter 3 Analysis of Original Steel Post
Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part
More 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 informationManual for Abaqus CAE Topology Optimization
Abaqus CAE access: Manual for Abaqus CAE Topology Optimization 1. Open Exceed ondemand Client -> login and pass 2FA 2. Select Desktop_Mode_Full_Screen (or other user preferred resolution) for XConfig and
More informationPrescribed Deformations
u Prescribed Deformations Outline 1 Description 2 Finite Element Model 2.1 Geometry Definition 2.2 Properties 2.3 Boundary Conditions 2.3.1 Constraints 2.3.2 Prescribed Deformation 2.4 Loads 2.4.1 Dead
More informationWORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14
WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.
More informationTutorial. Spring Foundation
Page i Preface This tutorial provides an example on how to model a spring foundation using BRIGADE/Plus. Page ii Contents 1 OVERVIEW... 1 2 GEOMETRY... 1 3 MATERIAL AND SECTION PROPERTIES... 2 4 STEP DEFINITION...
More information