Tutorial #3 LSDyna: Pop Can Crushing Analysis By C. Daley
|
|
- Emory Osborn Henry
- 6 years ago
- Views:
Transcription
1 Engineering 9093 Ice Class Ship Structures Tutorial #3 LSDyna: Pop Can Crushing Analysis By C. Daley Overview For a general introduction of LSDyna see Tut #1. Unlike most finite element programs LSDyna can easily model buckling events, such as occur when an empty pop can is crushed. In this lab we will model that situation. Learning Objectives The lab builds on the LSDyna features learned in Lab#1 and #2. In this lab we will model a rigid block moving as a ram (constrained rigid body motion). The ram will strike a complex shell object (a pop can) and crush and fold the aluminum shell. We will import and mesh the can geometry as a CAD file (a.stp file), and combine it with blocks meshed in LS-PrePost. This simulation will take much longer to solve than the previous models because there are more and smaller elements involved. We will see how to set an appropriate solution time to give good results without taking too long to solve. LSDYNA Model #3 Pop Can Crushing Step 1: describe and sketch the problem: In this third example we will model an aluminum pop can as it is crushed between a moving ram and a rigid base. The problem is sketched below Tut#3: LSDyna Can Crushing Analysis, page 1
2 The problem description is as follows: Geometry- Aluminum Can (elasto-plastic), Base and Ram: 0.08 x.08 x.02 m (rigid) Load: the ram moves at constant speed Supports: the base is fixed, the ram is moving in z only. Material: the can is Aluminum 3104-H19, with = 2720 kg/m 3, E = 69e9 Pa, y = 2.6e8 Pa, = 0.34, Et= 1e9 Pa, thickness m (est) the base and ram are rigid blocks (density and modulus of steel as before) Units: N, m, Pa, s Step 2: Create a CAD model of the pop can. Using the program Rhino, and a scaled photo of a pop can, create a can profile: Then using the Revolve tool in Rhino, create a can surface model; 9093 Tut#3: LSDyna Can Crushing Analysis, page 2
3 Then scale the surface (3D scale) down by 1000 and export the can as an.stp file: Can.stp. The scaling is done so the can is imported into LS-PrePost in units of meters. (Note: the Can.stp file is available for those who wish to skip the Rhino step). Step 3: estimate expected results: Step 4: open LS-PrePost How can this be done? ~40lb = 170 N? 1) First, Open LS-PrePost which should be on the desktop, with Icon or Step 5: Import the.stp file of the can and mesh it. 1) Click the File, Import, STEP File menu: which lets you open the Can.stp file. This should result in a screen like: 2) The next step is to mesh the can. Click on the Element and Mesh, then click the Auto Mesher button: which opens a dialog window to mesh a CAD object. You will also see a Sel. geom. window that allows you to select the objects for meshing. The quickest way to select the whole can is to click on in the Sel.geom window. The can will change color when it is all selected. Now hit the button in the Auto Mesher form to estimate the appropriate element size. In this case the result should look like: 9093 Tut#3: LSDyna Can Crushing Analysis, page 3
4 which indicates that the elements will be about 0.00 m. This shows us the CAD model has been imported in m units. Unfortunately this won't mesh, because this dialog only estimates the mesh to 2 decimal places. Instead type in the Elem Size box. Now hit the button and you will see a mesh superimposed on the can shape: With this you can now click and. The mesh is set. The can.stp file was created with the can base just slightly above the origin. This will be more obvious when the base and ram are created. Step 6: Create the base and ram blocks. 1) Click on the Element and Mesh, then click the Shape Mesher button: which opens a dialog window to mesh standard objects. In the Entity box at the top, select: Box_Solid and fill in the ranges for X,Y,Z, the number of divisions (elements) in Vx, Vy and Vz, and the TargetName, so it looks like this: 9093 Tut#3: LSDyna Can Crushing Analysis, page 4
5 Then press Create, Accept. Now make the ram block by just editing the Z range to be and 0.145, edit the Target Name to Ram. Then press Create, Accept and Done. At this point you should have a window that looks like: 9093 Tut#3: LSDyna Can Crushing Analysis, page 5
6 Step 7: Define the material properties 1) Click the model and part button: which will bring up a new set of icons. 2) Click the keyword manager button: which opens a dialog window to directly create keywords. At this point the model option is selected, and there are 3 categories of keyword already there (element, node and part). Note that there are 6383 elements, along with the 7464 nodes and 3 parts. If you wish to name or rename the parts, you can edit the part descriptions, hit Accept and the parts will be renamed. Select the option and the window will display all the possible keywords: 1) Click on the + to the left of MAT to open the material options: 2) Select and then click on near the top of the window. A Keyword Input Form will open to allow input of the properties for this material model: 9093 Tut#3: LSDyna Can Crushing Analysis, page 6
7 3) click on NewID and fill in the form so that it look like this; then press and then press. This material model describes elastoplastic behavior in aluminum. 4) Now Select and then click on near the top of the window. A Keyword Input Form will open to allow input of the properties for this material model: click on NewID and fill in the form so that it look like this; then press and then press. This material model is used for rigid materials, though it has the density of steel. Step 6: Define the section properties 9093 Tut#3: LSDyna Can Crushing Analysis, page 7
8 1) In LSDyna the section properties contain information about the element parameters and the type of physics employed. In the Keyword Manager window, scroll down until you see the Section Keyword. Click on the + and then select SHELL 2) Click on near the top of the window. A Keyword Input Form will open to allow input of the properties for this section model. click on NewID and fill in the form as follows: The form shows that the plate elements will have a thickness of m (80 m), that there are 5 integration points through the thickness (NIP=5) and the shear factor is then press and then press. After pressing Accept, you will see in the right hand space of the form. (Don't worry if the SECID number is different). 3) Now we need a SOLID section for the elements in the sphere. Under the SECTION Keyword, scroll down and select SOLID 9093 Tut#3: LSDyna Can Crushing Analysis, page 8
9 4) Click on near the top of the window. A Keyword Input Form will open to allow input of the properties for this section model. click on NewID and fill in the form as follows: The form only needs a TITLE. There is no other data to enter. then press and then press. Step 7: Apply the material and section properties to the model (to the 'Part') 1) In the Keyword Manager window, select the Part Keyword, press + and select Part: Then press. There are 2 Parts defined, but the Section and Material information are not yet linked to the parts (there are zeros under SECID and MID);. 2) Note that the 3 parts are listed in the upper right area of the form: This means that you are editing the PopCan. (If the names are different, you can edit the TITLE and hit Press the black dot to the right of SECID, and you see the following window open; 9093 Tut#3: LSDyna Can Crushing Analysis, page 9
10 Select and press Done. When you do the SECID is updated. Click on the black dot to the right of MID and select and press Done. then press ( Don't press ). We now have to apply the properties to the solid elements of the base and ram. 3) Select the part listed in the upper right area of the form: Press the black dot to the right of SECID, and you see the following window open; Select and press Done. When you do the SECID is updated. Click on the black dot to the right of MID and select and press Done. Now press. 4) Select the part listed in the upper right area of the form: Press the black dot to the right of SECID, and you see the following window open; Select and press Done. When you do the SECID is updated. Click on the black dot to the right of MID and select and press Done. Now press and now press. We now have a finite element model with material and section properties. Step 8: Apply boundary conditions (fix the base) Rather than using the Keyword Manager window, we will use the Entity Creation tool to fix the base. The Model and Part button already selected: Click on the Create Entity button. This will bring us an Entity Creation form. Select the + Boundary and then select Spc : Now change to Create mode by selecting 9093 Tut#3: LSDyna Can Crushing Analysis, page 10
11 Make sure the Set option selected and all 6 degrees of freedom selected: Now you need to select the nodes at the left end of the model. A Sel. Nodes dialog box should be open: with Pick selected. Select the ByPart option: Now select the base part. Now all nodes in the base are selected and the screen should look like; Now in the Entity Creation form you can hit 9093 Tut#3: LSDyna Can Crushing Analysis, page 11 : You should see that a new node set has been created: Now hit to close the entity creation form.
12 Step 9: Define a curve to specify the ram movement: Click the model and part button: and click the keyword manager button: Now Scroll to DEFINE, open it ( hit +) and select and then the key at the top. This will bring up a Keyword Input Form to create the curve. The form is initially blank. Hit NewID, give it the Title Ram Movement and with A1 and O1 both = 0.0 hit the button. Now edit the A1 and O1 boxes to 1 and 1, and hit again. Now edit the A1 and O1 boxes to 1.1 and 1, and hit Now the table will look like: again. The above defines a standard unit ramp. To have the ram move down by 0.12m in seconds, we need to scale the curve. Now edit the SFA and SFO boxes to and The form will now look like this: Hit and you will see in the right hand side of the form. To check the curve, hit the button to see the curve plotted. You should see: 9093 Tut#3: LSDyna Can Crushing Analysis, page 12
13 Step 10: Specify the ram movement: Click the model and part button: and click the Keyword Manager button: Select the + BOUNDARY Keyword and then scroll down to select and hit Hit NewID, give it the Title Ram Motion. Beside the PID box click on the black dot. Select RAM and press Under DOF select 3 to set z translation. Under VAD select 2 to specify displacement. Beside the LCID box click on the black dot. Select RAM MOVEMENT curve and press. Now press and now press. You can close the BOUNDARY keyword in the Keyword Manager window. Step 10: Specify the Contact model. We will use the simplest form of contact modeling. In the Keyword Manager, select Contact and then select the AUTOMATIC_SINGLE _SURFACE option. Hit and see the form. Just select NewID and fill in the Title with "Contact Model" Now press and now press Tut#3: LSDyna Can Crushing Analysis, page 13
14 Step 11: Specify the duration of the simulation. Return to the Keyword Manager and select Scroll down to find and then click Put in the ENDTIM box : hit and Step 12: Specify output frequency. Return to the Keyword Manager and select the DATABASE and BINARY_D3PLOT Keywords. and then click Specify an output timestep DT for the plot data of seconds (0.050ms) hit and In the Keyword Manager window hit to close it Step 13: Save the.k file Under the File menu select the Save Keyword As command and save the file as PopCan.k in its own folder (to keep the output files all in one place) Step 14: Run the LS-Dyna Analysis 1) Click on the LS-Dyna Manager Program, which opens the window.: 9093 Tut#3: LSDyna Can Crushing Analysis, page 14
15 In the top menu, select Solver and select Start LS-Dyna Analysis. Nest you see the input screen. Use the Browse button to select the PopCan.k file. By default the same folder as the.k file is in will be the folder where the output is sent. When the.k file is selected, press the RUN button. A winow will pop up showing the computation steps. In this case the elapsed time will be about 50 seconds. When finished is should say Normal termination : If we had set the run duration to one second, the run would have taken much longer. In the case of such a long run, you don't have to wait for the run to complete to know how long its going to take. When LSDyna is solving, the run steps are shown in the command window. You can press Control-C to halt the execution. Then you can enter sw2 and the program will restart and show an estimate for time to complete. In the case of the above model with a 1 second termination time the interupted command window looks like; 9093 Tut#3: LSDyna Can Crushing Analysis, page 15
16 This shows that estimated time to complete is 13 hrs and 17 minutes. This also shows that the time step is 1.97 E-07 seconds. In other words there are about 5 million time steps to be calculated in one second. And all 6383 elems have to be solved for each time step. No wonder this will take over 13 hrs. But we didn't need to take a whole second to crush the can. By crushing the can in seconds, we sped up the process by 200x and shortened the time to about 50 seconds. The question to consider is whether both 1 second and seconds constiture a quast-static analysis. How would you find out if this is the case? Step 15: Examine results of the LS-Dyna Analysis 1) Re-Open LS-PrePost. 2) From the File Menu, Select Open and LS-Dyna Binary Plot. 3) In the same folder as the.k file should be a file called d3plot - open it. Now you should see the screen as shown below. You can hit the Play button to annimate the bar over the.005 second of analysis. To See more data, hit the Post button select von Mises Stress and, then hit the Fringe Component, and the plot will become: 9093 Tut#3: LSDyna Can Crushing Analysis, page 16
17 Now you will see the animated stresses Tut#3: LSDyna Can Crushing Analysis, page 17
18 Self Study Exercises: Student: For each of these exercises, be prepared to show the instructor your results if asked. Exercise #1 Change the duration. Create a copy of the.k file in a new directory. Change the duration (in Termination and Curve keywords) to be 0.01 seconds. What is different? Ex#1 Initials of Instructor Exercise #2 Redo the analysis with a thicker can (double the thickness). What is different? Ex#2 Initials of Instructor 9093 Tut#3: LSDyna Can Crushing Analysis, page 18
Tut #2 LSDyna: Impact Analysis By C. Daley
Engineering 9093 Ice Class Ship Structures Tut #2 LSDyna: Impact Analysis By C. Daley Overview For a general introduction of LSDyna see Tut. #1. Unlike most finite element programs LSDyna can easily model
More informationTutorial #1 Introduction to LSDyna: Simple Cantilever By C. Daley
Engineering 9093 Ice Class Ship Structures Tutorial #1 Introduction to LSDyna: Simple Cantilever By C. Daley Overview LSDyna is a special type of finite element program produced by Livermore Software Technology
More informationTutorial 1 : Create an LS-DYNA input deck for a ball impacting a plate
Tutorial 1 : Create an LS-DYNA input deck for a ball impacting a plate Case description: Ball: solid elements, rigid material Plate: shell elements, edges constrained Ball Initial Velocity: 10mm/ms Files
More informationA GUIDE TO DEVELOP FEA MODEL. 2D Model (Shell Element) In LS-DYNA
A GUIDE TO DEVELOP FEA MODEL 2D Model (Shell Element) In LS-DYNA By Dr. Rakhmad Arief Siregar CAED Lab. Mechanical Eng. Program Universiti Malaysia Perlis Problem 1: Preprocessing by LS-PREPOST 2.1 1.
More informationIntroduction to LS-PrePost 4.0 (workshop) Quanqing Yan, Philip Ho, LSTC 2014
Introduction to LS-PrePost 4.0 (workshop) Quanqing Yan, Philip Ho, LSTC 04 Table of Contents SECTION WORKSHOPS Overview - General Operations Workshop Mesh Generation Workshop Pre-Processing Workshop 3-6
More informationTutorial 2 :Create an LS-DYNA input deck for a simple inflatable airbag
Tutorial 2 :Create an LS-DYNA input deck for a simple inflatable airbag Case description: Airbag: shell elements, fabric material Constraints: none Files required: curves.k Step 1: Create a circle 1. Geometry
More informationLab#5 Combined analysis types in ANSYS By C. Daley
Engineering 5003 - Ship Structures I Lab#5 Combined analysis types in ANSYS By C. Daley Overview In this lab we will model a simple pinned column using shell elements. Once again, we will use SpaceClaim
More informationIntroduction to LS-PrePost (workshops) Quanqing Yan, Philip Ho, LSTC 2017
Introduction to LS-PrePost (workshops) Quanqing Yan, Philip Ho, LSTC 07 Table of Contents SECTION WORKSHOPS Overview - General Operations Workshop Mesh Generation Workshop Pre-Processing Workshop --5 Post-Processing
More informationCHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA
DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation
More information2: Static analysis of a plate
2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors
More 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 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 informationFEA of Composites Classical Lamination Theory Example 1
FEA of Composites Classical Lamination Theory Example 1 22.514 Instructor: Professor James Sherwood Author: Dimitri Soteropoulos Revised by Jacob Wardell Problem Description: A four layer [0/90] s graphite-epoxy
More informationSDC. Engineering Analysis with COSMOSWorks. Paul M. Kurowski Ph.D., P.Eng. SolidWorks 2003 / COSMOSWorks 2003
Engineering Analysis with COSMOSWorks SolidWorks 2003 / COSMOSWorks 2003 Paul M. Kurowski Ph.D., P.Eng. SDC PUBLICATIONS Design Generator, Inc. Schroff Development Corporation www.schroff.com www.schroff-europe.com
More 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 informationExercise 2: Bike Frame Analysis
Exercise 2: Bike Frame Analysis This exercise will analyze a new, innovative mountain bike frame design under structural loads. The objective is to determine the maximum stresses in the frame due to the
More informationExercise 2: Bike Frame Analysis
Exercise 2: Bike Frame Analysis This exercise will analyze a new, innovative mountain bike frame design under structural loads. The objective is to determine the maximum stresses in the frame due to the
More informationSliding Block LESSON 26. Objectives: Demonstrate the use of Contact LBCs in a simple exercise.
LESSON 26 Sliding Block 5 Objectives: Demonstrate the use of Contact LBCs in a simple exercise. Present method for monitoring a non-linear analysis progress. 26-1 26-2 LESSON 26 Sliding Block Model Description:
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 information16 SW Simulation design resources
16 SW Simulation design resources 16.1 Introduction This is simply a restatement of the SW Simulation online design scenarios tutorial with a little more visual detail supplied on the various menu picks
More 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 informationEngineering Analysis with
Engineering Analysis with SolidWorks Simulation 2013 Paul M. Kurowski SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Visit the following websites
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 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 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 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 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 informationEngineering Analysis with SolidWorks Simulation 2012
Engineering Analysis with SolidWorks Simulation 2012 Paul M. Kurowski SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Visit the following websites
More informationExercise 9a - Analysis Setup and Loading
Exercise 9a - Analysis Setup and Loading This exercise will focus on setting up a model for analysis. At the end of this exercise, you will run an analysis in OptiStruct. While this exercise is focused
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 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 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 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 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 informationPro MECHANICA STRUCTURE WILDFIRE 4. ELEMENTS AND APPLICATIONS Part I. Yves Gagnon, M.A.Sc. Finite Element Analyst & Structural Consultant SDC
Pro MECHANICA STRUCTURE WILDFIRE 4 ELEMENTS AND APPLICATIONS Part I Yves Gagnon, M.A.Sc. Finite Element Analyst & Structural Consultant SDC PUBLICATIONS Schroff Development Corporation www.schroff.com
More informationHow to set up a 2D CFD case in LS-DYNA. Marcus Timgren DYNAmore Nordic
How to set up a 2D CFD case in LS-DYNA Marcus Timgren DYNAmore Nordic Upcoming webex The following Webex about the ICFD solver are scheduled. How to set up a 2D FSI case in LS-DYNA Jan 23 How to set up
More informationFree-Shape Optimization of a 3-D Bracket using the Free-shape Method
Free-Shape Optimization of a 3-D Bracket using the Free-shape Method In this exercise, shape optimization on a solid bracket model will be performed using the Free- Shape optimization method. The objective
More informationFINITE ELEMENT ANALYSIS OF A PLANAR TRUSS
FINITE ELEMENT ANALYSIS OF A PLANAR TRUSS Instructor: Professor James Sherwood Revised: Michael Schraiber, Dimitri Soteropoulos Programs Utilized: HyperMesh Desktop v12.0, OptiStruct, HyperView This tutorial
More informationCrashbox Tutorial. In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0
Crashbox Tutorial In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0 (Written by Moritz Guenther, student at Altair Engineering GmbH) 1 HyperMesh* 1. Start
More informationShell-to-Solid Element Connector(RSSCON)
WORKSHOP 11 Shell-to-Solid Element Connector(RSSCON) Solid Shell MSC.Nastran 105 Exercise Workbook 11-1 11-2 MSC.Nastran 105 Exercise Workbook WORKSHOP 11 Shell-to-Solid Element Connector The introduction
More informationExercise 1: Axle Structural Static Analysis
Exercise 1: Axle Structural Static Analysis The purpose of this exercise is to cover the basic functionality of the Mechanical Toolbar (MTB) in the context of performing an actual analysis. Details of
More 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 informationSpur Gears Static Stress Analysis with Linear Material Models
Exercise A Spur Gears Static Stress Analysis with Linear Material Models Beam and Brick Elements Objective: Geometry: Determine the stress distribution in the spur gears when a moment of 93.75 in-lb is
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 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 informationElasto-Plastic Deformation of a Thin Plate
WORKSHOP PROBLEM 6 Elasto-Plastic Deformation of a Thin Plate W P y L x P Objectives: Demonstrate the use of elasto-plastic material properties. Create an accurate deformation plot of the model. Create
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 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 informationME Week 12 Piston Mechanical Event Simulation
Introduction to Mechanical Event Simulation The purpose of this introduction to Mechanical Event Simulation (MES) project is to explorer the dynamic simulation environment of Autodesk Simulation. This
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 informationNormal Modes - Rigid Element Analysis with RBE2 and CONM2
APPENDIX A Normal Modes - Rigid Element Analysis with RBE2 and CONM2 T 1 Z R Y Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised
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 informationRigid Element Analysis with RBAR
WORKSHOP 4 Rigid Element Analysis with RBAR Y Objectives: Idealize the tube with QUAD4 elements. Use RBAR elements to model a rigid end. Produce a Nastran input file that represents the cylinder. Submit
More informationNormal Modes - Rigid Element Analysis with RBE2 and CONM2
APPENDIX A Normal Modes - Rigid Element Analysis with RBE2 and CONM2 T 1 Z R Y Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised
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 informationInterface with FE programs
Page 1 of 47 Interdisciplinary > RFlex > Flexible body Interface Interface with FE programs RecurDyn/RFlex can import FE model from ANSYS, NX/NASTRAN, MSC/NASTRAN and I-DEAS. Figure 1 RecurDyn/RFlex Interface
More informationQuarter Symmetry Tank Stress (Draft 4 Oct 24 06)
Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of
More informationThe part to be analyzed is the bracket from the tutorial of Chapter 3.
Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component
More informationStiffened Plate With Pressure Loading
Supplementary Exercise - 3 Stiffened Plate With Pressure Loading Objective: geometry and 1/4 symmetry finite element model. beam elements using shell element edges. MSC.Patran 301 Exercise Workbook Supp3-1
More informationNormal Modes - Rigid Element Analysis with RBE2 and CONM2
LESSON 16 Normal Modes - Rigid Element Analysis with RBE2 and CONM2 Y Y Z Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised of plate
More informationEngineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering
Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they
More 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 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 informationRevision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
More informationRecent developments in OASYS Primer
Recent developments in OASYS Primer October 2004 Miles Thornton Engineering consultancy 7000 staff worldwide Arup is our founder s name, Ove Arup Oasys = Ove Arup Systems 2004 Copyright by DYNAmore GmbH
More informationFEA TUTORIAL 2D STRESS ANALYSIS OF A THIN BAR (Using ProMechanica Wildfire 1.0)
FEA TUTORIAL 2D STRESS ANALYSIS OF A THIN BAR (Using ProMechanica Wildfire 1.0) Introduction: A simple 2D stress analysis of a thin bar with a hole will be performed using Pro/Mechanica. The bar will be
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 informationEngine Gasket Model Instructions
SOL 600 Engine Gasket Model Instructions Demonstrated:! Set up the Model Database! 3D Model Import from a MSC.Nastran BDF! Creation of Groups from Element Properties! Complete the Material Models! Import
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 informationPTC Newsletter January 14th, 2002
PTC Email Newsletter January 14th, 2002 PTC Product Focus: Pro/MECHANICA (Structure) Tip of the Week: Creating and using Rigid Connections Upcoming Events and Training Class Schedules PTC Product Focus:
More informationPlasticity Bending Machine Tutorial (FFlex)
Plasticity Bending Machine Tutorial (FFlex) Copyright 2018 FunctionBay, Inc. All rights reserved. User and training documentation from FunctionBay, Inc. is subjected to the copyright laws of the Republic
More informationFINITE ELEMENT ANALYSIS OF A PROPPED CANTILEVER BEAM
FINITE ELEMENT ANALYSIS OF A PROPPED CANTILEVER BEAM Problem Description: Instructor: Professor James Sherwood Revised: Venkat Putcha, Dimitri Soteropoulos Programs Utilized: HyperMesh Desktop 12.0, OptiStruct,
More informationBIRD STRIKE ANALYSIS ON AN AIRCRAFT LEADING EDGE USING SPH BIRD MODEL
BIRD STRIKE ANALYSIS ON AN AIRCRAFT LEADING EDGE USING SPH BIRD MODEL The front facing edges of an airplane, which include the wings, nose cone and engine, are more prone to bird strikes. In this tutorial,
More informationSolidWorks. An Overview of SolidWorks and Its Associated Analysis Programs
An Overview of SolidWorks and Its Associated Analysis Programs prepared by Prof. D. Xue University of Calgary SolidWorks - a solid modeling CAD tool. COSMOSWorks - a design analysis system fully integrated
More informationUsing MSC.Nastran for Explicit FEM Simulations
3. LS-DYNA Anwenderforum, Bamberg 2004 CAE / IT III Using MSC.Nastran for Explicit FEM Simulations Patrick Doelfs, Dr. Ingo Neubauer MSC.Software GmbH, D-81829 München, Patrick.Doelfs@mscsoftware.com Abstract:
More informationFinite Element Analysis Using Creo Simulate 4.0
Introduction to Finite Element Analysis Using Creo Simulate 4.0 Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following
More informationLearning Module 8 Shape Optimization
Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with
More 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 informationDYNAFORM Release Notes 7/2014
DYNAFORM 5.9.2 Release Notes 7/2014 Significant Enhancements 1. The new function for Auto-Position, automatically position blank and tools for multi-stages. 2. Automatic Iterative Trim Line Development
More informationFinite Element Method using Pro/ENGINEER and ANSYS
Finite Element Method using Pro/ENGINEER and ANSYS Notes by R.W. Toogood The transfer of a model from Pro/ENGINEER to ANSYS will be demonstrated here for a simple solid model. Model idealizations such
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 informationFINITE ELEMENT ANALYSIS OF A PROPPED CANTILEVER BEAM
FINITE ELEMENT ANALYSIS OF A PROPPED CANTILEVER BEAM Problem Description: Instructor: Professor James Sherwood Revised: Venkat Putcha, Dimitri Soteropoulos, Sanjay Nainani Programs Utilized: HyperMesh
More informationAutodesk Inventor 2019 and Engineering Graphics
Autodesk Inventor 2019 and Engineering Graphics An Integrated Approach Randy H. Shih SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the
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 informationMeta-model based optimization of spot-welded crash box using differential evolution algorithm
Meta-model based optimization of spot-welded crash box using differential evolution algorithm Abstract Ahmet Serdar Önal 1, Necmettin Kaya 2 1 Beyçelik Gestamp Kalip ve Oto Yan San. Paz. ve Tic. A.Ş, Bursa,
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 informationA Quadratic Pipe Element in LS-DYNA
A Quadratic Pipe Element in LS-DYNA Tobias Olsson, Daniel Hilding DYNAmore Nordic AB 1 Bacground Analysis of long piping structures can be challenging due to the enormous number of shell/solid elements
More informationFinite Element Analysis Using Pro/Engineer
Appendix A Finite Element Analysis Using Pro/Engineer A.1 INTRODUCTION Pro/ENGINEER is a three-dimensional product design tool that promotes practices in design while ensuring compliance with industry
More informationA plate with a hole is subjected to tension as shown: z p = 25.0 N/mm 2
Problem description A plate with a hole is subjected to tension as shown: z p = 25.0 N/mm 2 56 y All lengths in mm. Thickness =1mm E = 7.0 10 4 N/mm = 0.25 10 20 This is the same problem as problem 2.
More informationHelical Spring. Supplementary Exercise - 6. Objective: Develop model of a helical spring
Supplementary Exercise - 6 Helical Spring Objective: Develop model of a helical spring Perform a linear analysis to obtain displacements and stresses. MSC.Patran 301 Exercise Workbook Supp6-1 Supp6-2 MSC.Patran
More informationChapter 4 Feature Design Tree
4-1 Chapter 4 Feature Design Tree Understand Feature Interactions Use the FeatureManager Design Tree Modify and Update Feature Dimensions Perform History-Based Part Modifications Change the Names of Created
More informationRD-1070: Analysis of an Axi-symmetric Structure using RADIOSS
RADIOSS, MotionSolve, and OptiStruct RD-1070: Analysis of an Axi-symmetric Structure using RADIOSS In this tutorial, you will learn the method of modeling an axi- symmetry problem in RADIOSS. The figure
More informationTraining Guide TopSolid Fea
Training Guide i 2012, Missler Software. 7, Rue du Bois Sauvage F-91055 Evry, FRANCE Web: http://www.topsolid.com E-mail: info@topsolid.com All rights reserved. This information is subject to change without
More informationModeling and Analysis of Honeycomb Impact Attenuator
Modeling and Analysis of Honeycomb Impact Attenuator Preprocessor : Altair HyperMesh 14.0 Solver : Altair RADIOSS Postprocessor : Altair HyperView 1 An impact attenuator is a structure used to decelerate
More informationNeuerungen in LS-PrePost für das Pre- und Postprocessing von Composites
Neuerungen in LS-PrePost für das Pre- und Postprocessing von Composites Thomas Klöppel DYNAmore GmbH Stuttgart Anders Jernberg DYNAmore Nordic AB Linköping LS-PrePost für Composites - Thomas Klöppel -
More informationCoustyx Tutorial Indirect Model
Coustyx Tutorial Indirect Model 1 Introduction This tutorial is created to outline the steps required to compute radiated noise from a gearbox housing using Coustyx software. Detailed steps are given on
More informationAnalysis of a Tension Coupon
Y Z X Objectives: Manually define material and element properties. Manually create the geometry for the tension coupon using the given dimensions. Apply symmetric boundary constraints. Convert the pressure
More informationPTC Creo Simulate. Features and Specifications. Data Sheet
PTC Creo Simulate PTC Creo Simulate gives designers and engineers the power to evaluate structural and thermal product performance on your digital model before resorting to costly, time-consuming physical
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 informationCOMPUTATIONAL SIMULATION OF BLAST LOADING IN AN OPEN CYLINDER MODEL USING ANSYS AND LS-DYNA
COMPUTATIONAL SIMULATION OF BLAST LOADING IN AN OPEN CYLINDER MODEL USING ANSYS AND LS-DYNA Ramprashad Prabhakaran Graduate Student Department of Mechanical Engineering University of Nevada, Las Vegas
More information