Analysis of a Tension Coupon
|
|
|
- Leona Hawkins
- 5 years ago
- Views:
Transcription
1 WORKSHOP 14 Analysis of a Tension Coupon 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 loading into nodal forces. Run the analysis. Compare results. MSC.Nastran for Windows 101 Exercise Workbook 14-1
2 14-2 MSC.Nastran for Windows 101 Exercise Workbook
3 WORKSHOP 14 Analysis of a Tension Coupon Model Description: For the following problem, the user is expected to run the complete analysis and verify the results provided. This problem has the theoretical result. Users should not attempt these exercises unless they can construct geometry, create a finite element mesh, apply loads, material and element properties, run the analysis and postprocess the results or if they are willing to make a few mistakes and take a few wrong turns while trying. MSC.Nastran for Windows is intended to be self-explanatory, so it is okay to explore and try different techniques to complete this exercise, especially with a qualified instructor to help when you get lost. An experienced MSC.Nastran for Windows modeler should take no longer than 15 minutes to complete this problem, including the analysis. MSC.Nastran for Windows 101 Exercise Workbook 14-3
4 Figure Load Conditions psi psi y 10. z x Thickness =0.125 in. E = 30, 000, 000 psi ν = 0.3 Answer (Theory of Elasticity, Timoshenko & Goodier, 3rd edition, page 95): The answer given is the maximum at two points on the plate (Where?). P -- Þ K A f = 100. ( 4.3) σ xx = 430 psi Because of symmetry, the model simplifies into the model below psi MSC.Nastran for Windows 101 Exercise Workbook
5 WORKSHOP 14 Analysis of a Tension Coupon Exercise Procedure: 1. Start up MSC.Nastran for Windows V4.0 and begin to create a new model. Double click on the icon labeled MSC.Nastran for Windows V4.0. On the Open Model File form, select New Model. Open Model File: New Model 2. Create a material called mat_1. From the pulldown menu, select Model/Material. Model/Material... Title: Youngs Modulus: mat_1 30E6 Poisson s Ratio: 0.3 Cancel 3. Create a property called plate to apply to the members of the plate itself. From the pulldown menu, select Model/Property. Model/Property... Title: plate To select the material, click on the list icon next to the databox and select mat_1. Material: 1..mat_1 Thicknesses, Tavg or T1: Cancel MSC.Nastran for Windows 101 Exercise Workbook 14-5
6 4. Create the geometry for the inner circle. The model of this coupon is symmetrical in the x and y direction. Therefore, only a quarter of the geometry needs to be created. Tools/Advanced Geometry... Geometry Engine: Standard First, create 2 arcs with radii of 1 using the Geometry/Curve-Arc/ Radius-Start-End command. Geometry/Curve-Arc/Radius-Start-End CSys: 1..Basic Cylindrical Locate-Enter Location at Start of Arc. R: 1 T: 0 Z: 0 Locate-Enter Location at End of Arc. R: 1 T: 45 Z: 0 Radius: 1 Repeat the above steps to create a second curve using the following data...start.. R: 1 T: 45 Z: 0..End.. R: 1 T: 90 Z: 0 Radius: 1 Cancel To fit the display onto the screen, use the Autoscale feature. View/Autoscale <Ctrl+A> On your display, there should now be a quarter of a circle from 0 degrees to 90 degrees MSC.Nastran for Windows 101 Exercise Workbook
7 WORKSHOP 14 Analysis of a Tension Coupon Figure Create the geometry for the outer perimeter. Create two opposite edges using the Geometry/Curve-Line/ Project Points... command. Geometry/Curve-Line/Project Points... CSys: 0..Basic Rectangular...First Location... X: 5 Y: 0 Z: 0...Second Location... X: 5 Y: 2 Z: 0 Repeat the above steps to create the second line using the following data....first... X: 5 Y: 2 Z: 0...Second... X: 0 Y: 2 Z: 0 Cancel MSC.Nastran for Windows 101 Exercise Workbook 14-7
8 To fit the display onto the screen, use the Autoscale feature. View/Autoscale <Ctrl+A> The viewport should appear as shown. Figure Create the geometry for the surface of the plate. First, turn on the curve labels. View/Options... Options: Label Mode: <F6> Curve 1..ID Create 2 surfaces using the Geometry/Surface/Ruled command. Geometry/Surface/Ruled... From Curve: 2 To Curve: 4 From Curve: 1 To Curve: 3 Cancel When we created the surfaces, two coincident curves were generated along the common edge MSC.Nastran for Windows 101 Exercise Workbook
9 WORKSHOP 14 Analysis of a Tension Coupon Merge these curves. Tools/Check/Coincident Curves... Select All Options: Merge Coincident Entities Turn off the workplane. Tools/Workplane... Done View/Regenerate <Ctrl+G> Notice that there is now only one curve along the common edge. This will make it easier to apply the mesh control to the surfaces. 7. Define appropriate mesh size for critical edges. Draw Workplane It is very important to know the direction of each curve and line. The direction will determine the bias ratio of the mesh seeds. In steps 4 through 6, the geometry of this model was created so that the direction of the lines, curves and surfaces were pointing in the direction shown in Figure View/Options... <F6> Category: Options: (highlight) Parametric Directions: (highlight) Tools and View Style Curve and Surface Accuracy 1..Show Arrows MSC.Nastran for Windows 101 Exercise Workbook 14-9
10 Figure elem 4:1 10 elem 4:1 6 elem 1:1 10 elem 4:1 10 elem 4:1 10 elem 4:1 6 elem 1:1 Using the Mesh/Mesh Control/Size Along Curve... command, create the appropriate mesh seeds. The seeding varies depending on the Number of Elements and the density of the seeds set with the Bias inputs. Mesh/Mesh Control/Size Along Curve... <Select curve - ID #2, 4, 6, 8> Number of Elements 10 Node Spacing: Bias Factor: 4 Biased Small Elements at End <Select curve - ID # 5> Number of Elements 10 Node Spacing: Biased Bias Factor: 4 Small Elements at Start <Select curve - ID # 1, 3> Number of Elements MSC.Nastran for Windows 101 Exercise Workbook
11 WORKSHOP 14 Analysis of a Tension Coupon Node Spacing: Cancel Equal 8. Generate the finite elements. Mesh the two surfaces using the Mesh/Geometry/Surface... command. Mesh/Geometry/Surface... <select both surfaces +1, +2> Property: 1..plate 9. Remove coincident grids from the model. As you may have noticed on the screen, additional nodes were created while generating quad elements. To eliminate these coincident nodes, do the following: Tools/Check/Coincident Nodes... Select All When asked if it is to specify an additional range of nodes to merge, respond No. No Options: Merge Coincident Entities The message window should state that 11 Node(s) Merged. MSC.Nastran for Windows 101 Exercise Workbook 14-11
12 To better view the display and verify that duplicate nodes are deleted, do the following to remove the unnecessary labels. View/Options... <F6> Quick Options... Labels Off Done Node Category: Options: (highlight) Label Mode: Options: Label Mode: Category: Options: (highlight) Parametric Direction: Labels, Entities and Color Load-Force 1..Load Value Constraint 1..Degree of Freedom Tools and View Style Curve and Surface Accuracy 0..Off 10. Create the model constraints. Before creating the appropriate constraints, a constraint set needs to be created. Do so by performing the following: Model/Constraint/Set... Title: constraint This constraint set will have 3 different constraints MSC.Nastran for Windows 101 Exercise Workbook
13 WORKSHOP 14 Analysis of a Tension Coupon Figure 14.5 D A (X Sym) C (Fix TZ) B (Y Sym) Now define the first relevant constraint for the model. Use Figure 14.5 to identify appropriate curve selections. Model/Constraint/Nodal... Method^ on Curve <Select Curve 5 on the left edge. Box A in Figure 14.5> X Symmetry On the DOF box, TX, RY, and RZ should now have check marks. TX RY RZ Next, define the second relevant constraint for the model. Method^ on Curve <Select Curve 8 on the bottom edge. Box B in Figure 14.5> MSC.Nastran for Windows 101 Exercise Workbook 14-13
14 Y Symmetry On the DOF box, TY, RX, and RZ should now have check marks. TY RX RZ Finally, define the third relevant constraint for the model. <Select node 122 on the bottom left corner. Circle C in Figure14.5> On the DOF box, choose TZ to restrain movement in the Z direction. A warning message will appear: Selected concurrents already exist. to Overwrite (No = Combine)? Select NO to combine. No Cancel NOTE: This constraint is necessary to constrain the rigid body motion in and out of plane. 11. Create the loading conditions. Before creating the appropriate loading a load set needs to be created. Do so by performing the following: Model/Load/Set... TZ Title: tension MSC.Nastran for Windows 101 Exercise Workbook
15 WORKSHOP 14 Analysis of a Tension Coupon Since pressure is not an available option, the pressure must be converted into nodal forces and applied to the model. In this model, a 100 psi pressure force acting over the 0.25 in 2 (2 in x in) can be converted to a total equivalent nodal force of 25- lbs. Since we are going to distribute this force over 2 inches of edge length, the force per length will be 12.5 lbs/in. Note that when N4W writes to the.dat file, the 2 nodes on each corner will have lbs applied to them, while the 5 inner nodes will have lbs applied to them. Model/Load/On Curve... <Select Curve 3 on the right edge. Box D in Figure 14.5> (highlight) Force Per Length FX 12.5 Cancel To visualize nodal forces Model/Load/Expand... View/Regenerate <Ctrl+G> 12. Create the input file for analysis. File/Export/Analysis Model... Analysis Format/Type: 1..Static Change the directory to C: \temp. File Name: Write tension MSC.Nastran for Windows 101 Exercise Workbook 14-15
16 Run Analysis When asked to Save Model Now? Respond Yes. Yes When the MSC.Nastran manager is through running, MSC.Nastran for windows will be restored on your screen, and the Message Review form will appear. To read the messages, you could select Show Details. Since the analysis ran successfully, we will not bother with the details this time. Continue 13. View the results of the analysis. View the X Normal Stress Fringe Plot. View/Select... <F5> Contour Style: Deformed and Contour Data... Output Vectors/Contour: Contour Plate Top X Normal Stress From the Stress Scale, what is the maximum stress? Maximum Stress = Compare this value to the theoretical value. This concludes the exercise. File/Save File/Exit Max Average Nodal Stress MSC.Nastran for Windows 101 Exercise Workbook
Analysis 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
Rigid Element Analysis with RBE2 and CONM2
WORKSHOP 8 Rigid Element Analysis with RBE2 and CONM2 Y Z X Objectives: Create a geometric representation of a tube. Use the geometry model to define an analysis model comprised of plate elements. Idealize
Linear Static Analysis of a Simply-Supported Stiffened Plate
WORKSHOP 7 Linear Static Analysis of a Simply-Supported Stiffened Plate Objectives: Create a geometric representation of a stiffened plate. Use the geometry model to define an analysis model comprised
Simple Lumped Mass System
WORKSHOP 22 Simple Lumped Mass System Y X Objectives: Model a simple lumped mass system using beam elements and mass elements. Apply the proper constraints to the model to ensure stability during analysis.
Nonlinear Creep Analysis
WORKSHOP PROBLEM 7 Nonlinear Creep Analysis Objectives: Create the appropriate load cases for nonlinear static and nonlinear creep loads. Examine the strain for each subcase. Run an MSC/NASTRAN nonlinear
Scuba Tank: Solid Mesh
WORKSHOP 21a Scuba Tank: Solid Mesh Objectives: Create solid tank model. Evaluate Results. Remesh. Evaluate Results. MSC.Nastran for Windows 101 Exercise Workbook 21a-1 21a-2 MSC.Nastran for Windows 101
2-D Slideline Contact
WORKSHOP PROBLEM 9 2-D Slideline Contact Objectives: Demonstrate the use of slideline contact. Create the appropriate load cases, one with enforced displacement and the other without. Run an MSC/NASTRAN
Linear Buckling Analysis of a Plate
Workshop 9 Linear Buckling Analysis of a Plate Objectives Create a geometric representation of a plate. Apply a compression load to two apposite sides of the plate. Run a linear buckling analysis. 9-1
Linear Static Analysis for a 3-D Slideline Contact
WORKSHOP PROBLEM 10a Linear Static Analysis for a 3-D Slideline Contact Objectives: Demonstrate the use of slideline contact. Run an MSC/NASTRAN linear static analysis. Create an accurate deformation plot
Geometric Linear Analysis of a Cantilever Beam
WORKSHOP PROBLEM 2a Geometric Linear Analysis of a Cantilever Beam Objectives: Demonstrate the use of geometric linear analysis. Observe the behavior of the cantilever beam under four increasing load magnitudes.
Linear Buckling Load Analysis (without spring)
WORKSHOP PROBLEM 4a Linear Buckling Load Analysis (without spring) Objectives: Create and prepare the appropriate model for the analysis. Demonstrate the use of linear buckling analysis. MSC/NASTRAN for
Spring Element with Nonlinear Analysis Parameters (large displacements off)
WORKSHOP PROBLEM 1a Spring Element with Nonlinear Analysis Parameters (large displacements off) Objectives: Create a model of a simple rod and grounded spring system. Apply the appropriate constraints
Elasto-Plastic Deformation of a Truss Structure
WORKSHOP PROBLEM 8 Elasto-Plastic Deformation of a Truss Structure Objectives: Demonstrate the use of elastic-plastic material properties. Create an enforced displacement on the model. Run an MSC/NASTRAN
Creating Alternate Coordinate Frames
WORKSHOP 4 Creating Alternate Coordinate Frames 10 10 [ 23 34 0 ] Objectives: Create a geometric representation of a plate using a basic coordinate system as the reference and analysis coordinate system..
Directional Heat Loads
LESSON 4 Directional Heat Loads Objectives: Create a geometric model of a cylinder. Apply ambient radiation to space and a directional heat flux to the model. Run a steady-state heat transfer analysis
Varying Thickness-Tapered
APPENDIX B Varying Thickness-Tapered Objectives: Create a geometric representation of a flat rectangular plate. Use the geometry model to define an analysis model comprised of plate elements. Use a function
Modal Analysis of A Flat Plate using Static Reduction
WORKSHOP PROBLEM 2 Modal Analysis of A Flat Plate using Static Reduction Objectives Reduce the dynamic math model, created in Workshop 1, to one with fewer degrees of freedom. Apply the static reduction
Free Convection on a Printed Circuit Board
LESSON 6 Free Convection on a Printed Circuit Board Objectives: Create a geometric representation of a printed circuit board. Apply thermal loading of free convection and heat fluxes to the model. Run
Radiation Enclosures
LESSON 3 Radiation Enclosures Objectives: Create a geometric representation of three plates. Aply a thermal load of heat flux to a patch in the middle surface. Apply thermal load of shaded radiation to
Direct Transient Response with Base Excitation
WORKSHOP PROBLEM 7 Direct Transient Response with Base Excitation Z Y X Objectives Create a geometric representation of a flat rectangular plate. Use the geometry model to define an analysis model comprised
Forced Convection on a Printed Circuit Board
LESSON 7 Forced Convection on a Printed Circuit Board Objectives: Create a geometric representation of a plate. Apply thermal loading of forced convection and heat fluxes to the model. Run a steady-state
The 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
Spring Element with Nonlinear Analysis Parameters (Multi-step Analysis)
WORKSHOP PROBLEM 1c Spring Element with Nonlinear Analysis Parameters (Multi-step Analysis) Objectives: Import the model from the previous exercise. Apply incremental load through multiple subcases. Submit
Modal Transient Response Analysis
WORKSHOP PROBLEM 4 Modal Transient Response Analysis Z Y X Objectives Create a geometric representation of a flat rectangular plate. Use the geometry model to define an analysis model comprised of plate
Rigid 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
Shell-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
6-1. Simple Solid BASIC ANALYSIS. Simple Solid
6-1 6 BASIC ANALYSIS 6-2 Model Description: This example is used to show some simple solid modeling while keeping the number of nodes of the solid mesh under the 300 node limit of the demonstration version.
Mesh Cleanup WORKSHOP 10. Objectives. Model Description: Mesh Cleanup. Import an ACIS geometry file. Mesh the part.
Objectives Import an ACIS geometry file. Mesh the part. Find and delete collapsed elements. Remesh the part. MSC.Nastran for Windows 101 Exercise Workbook 10-1 Model Description: Solids created in CAD
MAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1
Instructions MAE 323 Lab Instructions 1 Problem Definition Determine how different element types perform for modeling a cylindrical pressure vessel over a wide range of r/t ratios, and how the hoop stress
Linear 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
Spatial Variation of Physical Properties
LESSON 5 Spatial Variation of Physical Properties Aluminum Steel 45 Radius 1 Radius 3 Radius 4 Objective: To model the variation of physical properties as a function of spatial coordinates. MSC/NASTRAN
Spatial Variation of Physical Properties
LESSON 13 Spatial Variation of Physical Properties Aluminum Steel 45 Radius 1 Radius 3 Radius 4 Objective: To model the variation of physical properties as a function of spatial coordinates. PATRAN301ExericseWorkbook-Release7.5
Normal 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
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
Transient Response of a Rocket
Transient Response of a Rocket 100 Force 0 1.0 1.001 3.0 Time Objectives: Develope a finite element model that represents an axial force (thrust) applied to a rocket over time. Perform a linear transient
FEMAP Tutorial 2. Figure 1: Bar with defined dimensions
FEMAP Tutorial 2 Consider a cantilevered beam with a vertical force applied to the right end. We will utilize the same geometry as the previous tutorial that considered an axial loading. Thus, this tutorial
Normal 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
Post-Buckling Analysis of a Thin Plate
LESSON 13b Post-Buckling Analysis of a Thin Plate Objectives: Construct a thin plate (with slight imperfection) Place an axial load on the plate. Run an Advanced FEA nonlinear static analysis in order
Normal 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
Sliding 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,
Helical 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
Stiffened 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
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
Using Groups and Lists
LESSON 15 Using Groups and Lists Objectives: Build a finite element model that includes element properties and boundary conditions. Use lists to identify parts of the model with specified attributes. Explore
Elastic Stability of a Plate
WORKSHOP PROBLEM 7 Elastic Stability of a Plate Objectives Produce a Nastran input file. Submit the file for analysis in MSC/NASTRAN. Find the first five natural modes of the plate. MSC/NASTRAN 101 Exercise
FEA 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
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
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.
Elasto-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
Linear Static Analysis of a Spring Element (CELAS)
Linear Static Analysis of a Spring Element (CELAS) Objectives: Modify nodal analysis and nodal definition coordinate systems to reference a local coordinate system. Define bar elements connected with a
Modal Analysis of a Flat Plate
WORKSHOP 1 Modal Analysis of a Flat Plate Objectives Produce a MSC.Nastran input file. Submit the file for analysis in MSC.Nastran. Find the first five natural frequencies and mode shapes of the flat plate.
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
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
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
Restarting a Linear Static Analysis of a Simply- Supported Stiffened Plate
WORKSHOP 15 Restarting a Linear Static Analysis of a Simply- Supported Stiffened Plate Objectives: Submit a job to MSC.Nastran for analysis and save the restart files. (SCR = NO) Perform a restart on a
Shear and Moment Reactions - Linear Static Analysis with RBE3
WORKSHOP 10a Shear and Moment Reactions - Linear Static Analysis with RBE3 250 10 15 M16x2 bolts F = 16 kn C B O 60 60 200 D A Objectives: 75 75 50 300 Create a geometric representation of the bolts. Use
Sliding 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:
Rigid Element Analysis with RBE2 and CONM2
WORKSHOP PROBLEM 5 Rigid Element Analysis with RBE2 and CONM2 Y Y Z Z X Objectives: Idealize a rigid end using RBE2 elements. Define a concentrated mass, to represent the weight of the rigid enclosure
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
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
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
Quarter 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
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.
Load Lug Model EXERCISE 6. Objective: Write a function to apply the loads and element properties to the finite element mesh of the lug.
EXERCISE 6 Load Lug Model Objective: Write a function to apply the loads and element properties to the finite element mesh of the lug. PATRAN 304 Exercise Workbook 6-1 6-2 PATRAN 304 Exercise Workbook
Cylinder with T-Beam Stiffeners
LESSON 17 Cylinder with T-Beam Stiffeners X Y Objectives: Create a cylinder and apply loads. Use the beam library to add stiffeners to the cylinder. PATRAN 302 Exercise Workbook - Release 8.0 17-1 17-2
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
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
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:
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
APPENDIX B. PBEAML Exercise. MSC.Nastran 105 Exercise Workbook B-1
APPENDIX B PBEAML Exercise MSC.Nastran 105 Exercise Workbook B-1 B-2 MSC.Nastran 105 Exercise Workbook APPENDIX B PBEAML Exercise Exercise Procedure: 1. Create a new database called pbeam.db. File/New...
Engine 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
Heat Transfer Analysis of a Pipe
LESSON 25 Heat Transfer Analysis of a Pipe 3 Fluid 800 Ambient Temperture Temperture, C 800 500 2 Dia Fluid Ambient 10 20 30 40 Time, s Objectives: Transient Heat Transfer Analysis Model Convection, Conduction
FINITE 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,
Finite Element Model of a 3-D Clevis
LESSON 4 Finite Element Model of a 3-D Clevis Objectives: Apply a nonuniform mesh seed near a critical location of the model. Apply a global mesh to the seeded model. PATRAN 303 Exercise Workbook - Release
Linear Static Analysis of a Simply-Supported Truss
WORKSHOP PROBLEM 2 Linear Static Analysis of a Simply-Supported Truss Objectives: Define a set of material properties using the beam library. Perform a static analysis of a truss under 3 separate loading
Exercise 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
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
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
Modal Analysis of Interpolation Constraint Elements and Concentrated Mass
APPENDIX B Modal Analysis of Interpolation Constraint Elements and Concentrated Mass Y Y Z Z X Objectives: Utilize the analysis model created in a previous exercise. Run an MSC.Nastran modal analysis with
MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook
MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook P3*V8.0*Z*Z*Z*SM-PAT325-WBK - 1 - - 2 - Table of Contents Page 1 Composite Model of Loaded Flat Plate 2 Failure Criteria for Flat Plate 3 Making Plies
FINITE 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
RD-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
Mass Properties Calculations
LESSON 15 Mass Properties Calculations Objectives Import a unigraphics express file and apply mass properties to the propeller. PAT302 Exercise Workbook MSC/PATRAN Version 8.0 15-1 15-2 PAT302 Exercise
Linear Static Analysis of a Simply-Supported Truss
LESSON 8 Linear Static Analysis of a Simply-Supported Truss Objectives: Create a finite element model by explicitly defining node locations and element connectivities. Define a MSC/NASTRAN analysis model
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
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
ANSYS 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
ES 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.
WORKSHOP 33 A1 A2 A1. Subcase 1 4 Subcase 2 X: -16,000 lbs. X: 16,000 lbs Y: -12,000 lbs. Y: -12,000 lbs. Objectives:
WORKSHOP 33 y 2 x 1 3 A1 A2 A1 1 2 3 Subcase 1 4 Subcase 2 X: -16,000 lbs X: 16,000 lbs Y: -12,000 lbs Y: -12,000 lbs Objectives: Optimize the following three-bar truss problem subject to static loading.
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
CATIA V5 FEA Tutorials Release 14
CATIA V5 FEA Tutorials Release 14 Nader G. Zamani University of Windsor SDC PUBLICATIONS Schroff Development Corporation www.schroff.com www.schroff-europe.com CATIA V5 FEA Tutorials 2-1 Chapter 2 Analysis
ME 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
Finite Element Model
LESSON 9 Finite Element Model Objectives: Build an initial surface mesh that will be used as a pattern to create the final 1, 2 and 3D mesh. Edit and smooth the mesh. Build a finite element model by sweeping
Manual for Computational Exercises
Manual for the computational exercise in TMM4160 Fracture Mechanics Page 1 of 32 TMM4160 Fracture Mechanics Manual for Computational Exercises Version 3.0 Zhiliang Zhang Dept. of Structural Engineering
ixcube 4-10 Brief introduction for membrane and cable systems.
ixcube 4-10 Brief introduction for membrane and cable systems. ixcube is the evolution of 20 years of R&D in the field of membrane structures so it takes a while to understand the basic features. You must
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,
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
Spur 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
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
Nonlinear Creep Analysis
WORKSHOP PROBLEM 7 Nonlinear Creep Analysis Objectives: Demonstrate the use of creep material properties. Examine the strain for each subcase. Create an XY plot of Load vs. Displacement for all the subcases.