Scuba Tank: Solid Mesh
|
|
|
- Octavia Watson
- 6 years ago
- Views:
Transcription
1 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
2 21a-2 MSC.Nastran for Windows 101 Exercise Workbook
3 WORKSHOP 21a Scuba Tank: Solid Mesh Model Description: This exercise will import a partially created geometric model of a scubatank. A quarter symmetry finite element model will be constructed and analyzed. These results will be evaluated, then a second mesh will be generated and analyzed. Figure 21a.1 - Model Geometry MSC.Nastran for Windows 101 Exercise Workbook 21a-3
4 Suggested Exercise Steps: Import the file tank_outline.neu Complete the quarter tank geometric model. Create the material and property. Save these data in a neutral file for later use. Solid mesh the model. Apply loads and constraints. Run anaylsis and evaluate results. Create a new model with a finer mesh. Run analysis and evaluate results. 21a-4 MSC.Nastran for Windows 101 Exercise Workbook
5 WORKSHOP 21a Scuba Tank: Solid Mesh 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: Tools/Advanced Geometry... Geometry Engine: New Model Standard 2. The cross-section geometry has already been created and stored in a FEMAP Neutral file. File/Import/FEMAP Neutral... Change directory to c:\training\examples. File name: Open tank_outline.neu The workplane will not be necessary. Right Click on screen to invoke the pop up menu. Workplane... Uncheck Draw Workplane. Draw Workplane Done 3. Rotate the model. View/Rotate... <F8> X: 0 MSC.Nastran for Windows 101 Exercise Workbook 21a-5
6 Y: -90 Z: 90 View/Autoscale <Ctrl+A> Figure 21a.2 4. Turn on Curve IDs. View/Options... Options: Label Mode: <F6> Curve 1..ID 21a-6 MSC.Nastran for Windows 101 Exercise Workbook
7 WORKSHOP 21a Scuba Tank: Solid Mesh Figure 21a.3 5. Create several ruled surfaces using the following curve pairs: Geometry/Surface/Ruled... From Curve: 21 To Curve: 22 Continue for the following combinations: From Curve: To Curve: Cancel MSC.Nastran for Windows 101 Exercise Workbook 21a-7
8 Figure 21a.4 6. Merge coincident curves. Tools/Check/Coincident Curves... Select All Options: Merge Coincident Entities View/Redraw... <Ctrl+D> 7. Revolve these surfaces to generate volume geometry. Geometry/Volume/Revolve... Select All Methods ^ Global Axis Direction: Positive Z Axis Rotation Angle: 90 21a-8 MSC.Nastran for Windows 101 Exercise Workbook
9 WORKSHOP 21a Scuba Tank: Solid Mesh Cancel 8. Reposition volume. View/Rotate... <F8> X: 30 Y: 30 Z: 90 Figure 21a.5 The geometry is now complete. 9. Define a material for the model. Model/Material... Load... Library Entry: 17-4PH Stainless H1025 MSC.Nastran for Windows 101 Exercise Workbook 21a-9
10 Cancel 10. Define the model property. Model/Property... Elem/Property Type... Volume Elements: Title: Material: Material Axes: Cancel Solid Solid_Stainless PH Stainless H Basic Cylindrical Align to CSys 11. Apply mesh control. Mesh/Mesh Control/Size Along Curve... Select all 14 curves radial curves (Curves 60, 59, 66, 61, 58, 65, 53, 63, 62, 54, 64, 57, 56, 55) Number of Elements: 6 Cancel View/Rotate... <F8> X: 30 Y: 30 Z: a-10 MSC.Nastran for Windows 101 Exercise Workbook
11 WORKSHOP 21a Scuba Tank: Solid Mesh 12. Turn off curve labels. View/Options... Category: Options: Label Mode: Labels, Entities and Color Curve 0..No Labels View/Magnify... Fill View Figure 21a Save this model to a neutral file. This geometry will be used later to generate a finer mesh model to compare results. File/Export/FEMAP Neutral... File Name: Write tank_quarter.neu MSC.Nastran for Windows 101 Exercise Workbook 21a-11
12 14. Mesh the geometry. Mesh/Geometry/Volume... Select All Property: Node Param... Output Coordinate System: 1..Solid Stainless 1..Basic Cylindrical Figure 21a Equivalence the finite element mesh. Tools/Check/Coincident Nodes... Select All No Options: Merge Coincident Entities 21a-12 MSC.Nastran for Windows 101 Exercise Workbook
13 WORKSHOP 21a Scuba Tank: Solid Mesh Click the Quick Options icon and turn off the geometry. Quick Options Geometry Off Done Figure 21a.8 View/Select... <F5> Model Style: Free Edge MSC.Nastran for Windows 101 Exercise Workbook 21a-13
14 Figure 21a.9 View/Select... <F5> Model Style: Full Hidden Line Figure 21a.10 21a-14 MSC.Nastran for Windows 101 Exercise Workbook
15 WORKSHOP 21a Scuba Tank: Solid Mesh 16. Apply constraints to the model. Model/Constraint/Set... <Shift+F2> Title: Symmetric Apply symmetric constraints. Model/Constraint/Nodal... Method ^ on Surface ID: 1 to: 14 by: 1 DOF: TT Select Node 44 (see Fig. 21a.11) Figure 21a DOF: TR MSC.Nastran for Windows 101 Exercise Workbook 21a-15
16 When asked, to Overwrite (No=Combine)?, select No. No Now restrain nodes on the opening in the z-direction. Method ^ on Surface Select Surface 34 (see Fig. 21a.12) Figure 21a DOF: TZ No Cancel 17. Create a load of 500 psi internal pressure. Model/Load/Set... <Ctrl+F2> Title: 5_Ksi 21a-16 MSC.Nastran for Windows 101 Exercise Workbook
17 WORKSHOP 21a Scuba Tank: Solid Mesh Model/Load/Elemental... Select All (highlight) Pressure Pressure: 5000 Method: Adjacent Faces Pick a face element on the inside face of the tank. Element: 100 Tolerance: 45 Face: 5 Cancel Figure 21a.13 MSC.Nastran for Windows 101 Exercise Workbook 21a-17
18 18. Run an analysis. File/Export/Analysis Model... <Ctrl+T> Type: File name: Write When the MSC.Nastran Manager is through running, MSC.Nastran will be restored on your screen, and the Message Review form will appear. To read the message(s), you could select Show Details. Since the analysis ran successfully, we will not bother with the details this time. 19. Review results. 1..Static tank_course Additional Info: Run Analysis Output Types: Yes File name: Save Continue 2..Displacements and Stresses tank_course Clean up the viewscreen by clicking on the following icon: Quick Options All Entities Off Draw: Element Done View/Select... <F5> Deformed Style: Contour Style: Deform and Contour Data... Deform Contour 21a-18 MSC.Nastran for Windows 101 Exercise Workbook
19 WORKSHOP 21a Scuba Tank: Solid Mesh Figure 21a.14 View/Select... <F5> Deformed Style: Contour Style: Deform and Contour Data... Contour: View/Select... <F5> Deform and Contour Data... Contour: None - Model Only Contour Solid X Normal Stress Solid Y Normal Stress Model/Output/Error Estimate... Output Vector: Solid Von MisesStresses MSC.Nastran for Windows 101 Exercise Workbook 21a-19
20 View/Select... <F5> Deform and Contour Data... Output Vector: ERROR ESTIMATE Now a finer mesh model will be created. File/New... Yes Tools/Advanced Geometry... Geometry Engine: Standard 21. The quarter tank geometry was created and stored in a FEMAP Neutral file in the first part of this exercise. File/Import/FEMAP Neutral... Change directory to c:\mscn4w40\examples. File name: Open tank_quarter.neu 22. Mesh the geometry. Mesh/Mesh Control/ Default Size... Min Elem: 6 View/Options... <F6> Category: Options: Surface Divisions: Tools and View Style Curve and Surface Accuracy 2..Show Mesh Size 21a-20 MSC.Nastran for Windows 101 Exercise Workbook
21 WORKSHOP 21a Scuba Tank: Solid Mesh Figure 21a Apply mesh control on surfaces.. Mesh/Mesh Control/Mapped Divisions on Surface... Select Surfaces 1 and 8 (see Fig. 21a.15) s: t: Number of Elements: 16 6 Bias: 1 1 Select Surfaces 5 and 12 (see Fig. 21a.15) s: t: MSC.Nastran for Windows 101 Exercise Workbook 21a-21
22 Number of Elements: 24 6 Bias: 1 1 Cancel 24. Apply a mesh control along curves. Mesh/Mesh Control/Size Along Curve... Select Curves 19, 20, 44, and 45 (see Fig. 21a.15) Mesh Size: Number of Elements 36 Node Spacing: Biased Bias Factor: 8 Node Spacing: Small Elements at Both Ends Cancel Mesh/Geometry/Volume... Select All Property: Node Param.. Output Coordinate System: CSys: 1..Solid Stainless 1..Basic Cylindrical 1..Basic Cylindrical 25. Equivalence the finite element mesh. Tools/Check/Coincident Nodes... Select All 21a-22 MSC.Nastran for Windows 101 Exercise Workbook
23 WORKSHOP 21a Scuba Tank: Solid Mesh No Options: Merge Coincident Entities View/Select... <F5> Model Style: View/Select... <F5> Model Style: Free Edge Full Hidden Line Click the Quick Options icon and turn off the geometry. Quick Options Draw: Node Geometry Off Done 26. Apply constraints to model. Model/Constraint/Set... <Shift+F2> Title: Symmetric Model/Constraint/Nodal... Method ^ on Surface ID: 1 to: 14 by: 1 DOF: TT MSC.Nastran for Windows 101 Exercise Workbook 21a-23
24 Method ^ on Surface Select Surface 34 (see Fig. 21a.16) Figure 21a DOF: TZ No Method ^ on Curve Select Curve 5 (see Fig. 21a.16) DOF: TR No Cancel 21a-24 MSC.Nastran for Windows 101 Exercise Workbook
25 WORKSHOP 21a Scuba Tank: Solid Mesh Click the Quick Options icon. Quick Options Draw: Constraint Done 27. Create loads. Model/Load/Set... <Ctrl+F2> Title: 5_Ksi Model/Load/Elemental... Select All (highlight) Pressure Pressure: 5000 Method: Adjacent Faces Select and element face on the inside face of the tank. Element: 1640 Tolerance: 20 Face: 5 Cancel Click the Quick Options icon and turn off the geometry. Quick Options All Entities Off Draw: Element MSC.Nastran for Windows 101 Exercise Workbook 21a-25
26 Done Figure 21a Run analysis. File/Export/Analysis Model... <Ctrl+T> File Name: 1..Static File Name: tank_fine Write Additional Info: Run Analysis Output Types: 2..Displacements and Stresses Yes File Name: tank_fine Save 21a-26 MSC.Nastran for Windows 101 Exercise Workbook
27 WORKSHOP 21a Scuba Tank: Solid Mesh When the MSC.Nastran Manager is through running, MSC.Nastran will be restored on your screen, and the Message Review form will appear. To read the message(s), you could select Show Details. Since the analysis ran successfully, we will not bother with the details this time. Continue 29. Review and compare results. View/Select... <F5> Deformed Style: Contour Style: Deform and Contour Data... View/Select... <F5> Deformed Style: Contour Style: Deform and Contour Data... Contour: View/Select... <F5> Deform and Contour Data... Contour: Deform Contour None - Model Only Contour Solid X Normal Stress Solid Y Normal Stress Model/Output/Error Estimate... Output Vector: Solid Von MisesStresses View/Select... <F5> MSC.Nastran for Windows 101 Exercise Workbook 21a-27
28 Deform and Contour Data... Output Vector: ERROR ESTIMATE This concludes the exercise. File/Save File/Exit 21a-28 MSC.Nastran for Windows 101 Exercise Workbook
Analysis of a Tension Coupon
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
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
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
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
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
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.
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
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
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.
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
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
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
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
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
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
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
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
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
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
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
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
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..
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
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
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.
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
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
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
Importing Geometry from an IGES file
WORKSHOP 2 Importing Geometry from an IGES file Objectives: Import geometry from an IGES file. Create a solid from curves and surfaces. Tet mesh the solid. MSC.Patran 301 Exercise Workbook 2-1 2-2 MSC.Patran
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
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
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
Projected Coordinate Systems
LESSON 8 Projected Coordinate Systems Objectives: To become familiar with the difference between Global and Projected-Global coordinate systems. To realize the importance of both coordinate systems. PATRAN
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
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
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
Importing Geometry from an IGES file
LESSON 2 Importing Geometry from an IGES file Objectives: Import geometry from an IGES file. Create a solid from curves and surfaces. Tet mesh the solid. PATRAN 301 Exercise Workbook - Release 7.5 2-1
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
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,
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
Post Processing of Displacement Results
WORKSHOP 16 Post Processing of Displacement Results Objectives: Examine the deformation of the MSC.Nastran model to evaluate the validity of the assumptions made in the creation of the mesh density and
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
EXERCISE 4. Create Lug Geometry. Objective: Write a function to create the geometry of the lug. PATRAN 304 Exercise Workbook 4-1
EXERCISE 4 Create Lug Geometry Objective: Write a function to create the geometry of the lug. PATRAN 304 Exercise Workbook 4-1 4-2 PATRAN 304 Exercise Workbook EXERCISE 4 Create Lug Geometry Exercise Description:
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
Projected Coordinate Systems
LESSON 16 Projected Coordinate Systems Objectives: To become familiar with the difference between Global and Projected-Global coordinate systems. To realize the importance of both coordinate systems. PATRAN
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
Post Processing of Displacement Results
LESSON 16 Post Processing of Displacement Results Objectives: Examine the deformation of the MSC/NASTRAN model to evaluate the validity of the assumptions made in the creation of the mesh density and selection
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
Lesson 25 Combining FEM Models
Lesson 25 Combining FEM Models Purpose This lesson provides an overview of combining models Finite Elements Models with Femap Topics Femap Neutral files The Select Tool File, Merge command Femap 101 for
Importing Results using a Results Template
LESSON 15 Importing Results using a Results Template Objectives: Write a custom nodal and displacement results template. Import a Patran 2.5 Neutral File model. Import a Patran 2.5 Results File. Perform
Importing a PATRAN 2.5 Model into P3
LESSON 1 Importing a PATRAN 2.5 Model into P3 Objectives: Read a PATRAN 2.5 neutral file into P3. Import PATRAN 2.5 result files into your P3 database. Work with multiple load cases. PATRAN 303 Exercise
Post Processing of Stress Results
LESSON 7 Post Processing of Stress Results Objectives: To post-process stress results from MSC/NASTRAN. To use MSC/PATRAN to create fill and fringe plots to determine if the analyzed part will meet a customerdefined
Post-Processing Static Results of a Space Satellite
LESSON 7 Post-Processing Static Results of a Space Satellite 3.84+05 3.58+05 3.33+05 3.07+05 2.82+05 3.84+05 2.56+05 2.30+05 2.05+05 1.79+05 1.54+05 1.28+05 1.02+05 7.68+04 0. 5.12+04 Z Y X Objectives:
Composite Trimmed Surfaces
LESSON 4 Composite Trimmed Surfaces Y Objectives: Import a CAD model into a database. Repair disjointed surfaces by creating composite surfaces. Mesh the newly created composite surfaces PATRAN 302 Exercise
FEMAP v New Features and Corrections Updates and Enhancements
FEMAP v11.0.1 New Features and Corrections Updates and Enhancements Connection Properties, Regions, and Connectors Geometry Model, Delete, Mesh now automatically deletes any Connection Regions where all
Load Analysis of a Beam (using a point force and moment)
WORKSHOP 13a Load Analysis of a Beam (using a point force and moment) 100 lbs Y Z X Objectives: Construct a 1d representation of a beam. Account for induced moments from an off-center compressive load
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
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
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:
Post Processing of Stress Results With Results
LESSON 10 Post Processing of Stress Results With Results Objectives: To post-process stress results from MSC/NASTRAN. To use MSC/PATRAN to create fill and fringe plots to determine if the analyzed part
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
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.
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
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
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
CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the
WORKSHOP 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.
Transient and Modal Animation
WORKSHOP 20 Transient and Modal Objectives: Introduce the user to insight animation tools. Perform standard and quick modal animation. Perform transient animation. MSC.Patran 301 Exercise Workbook 20-1
Problem 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
ANSYS AIM Tutorial Stepped Shaft in Axial Tension
ANSYS AIM Tutorial Stepped Shaft in Axial Tension Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Contents: Problem Specification 3 Learning Goals 4 Pre-Analysis & Start Up 5 Calculation
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
Similar Pulley Wheel Description J.E. Akin, Rice University
Similar Pulley Wheel Description J.E. Akin, Rice University The SolidWorks simulation tutorial on the analysis of an assembly suggested noting another type of boundary condition that is not illustrated
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...
Table of Contents Memory Management... 3 Results Enveloping... 5 Set Random Property Colors... 8 Model Box Extend Merge Mesh...
1 Table of Contents Memory Management... 3 Results Enveloping... 5 Set Random Property Colors... 8 Model Box... 11 Extend Merge Mesh... 13 NonManifold Add... 16 Element Visual Inspection... 18 Graphical
Post Processing of Results
LESSON 22 Post Processing of Results Objectives: Combine result cases. Use fringe plot options to more accurately look at stress fringe plots. Use xy plots to examine stresses at specific sections. Perform
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
Post-Processing Modal Results of a Space Satellite
LESSON 8 Post-Processing Modal Results of a Space Satellite 30000 7.61+00 5.39+00 30002 30001 mode 1 : Max 5.39+00 @Nd 977 Objectives: Post-process model results from an DB file. View and animate the eigenvector
Imported Geometry Cleaning
LESSON 8 Imported Geometry Cleaning Objectives: Import CAD geometry. Identify problems with imported geometry. Fix geometry for the purpose of meshing. PATRAN 302 Exercise Workbook - Release 8.0 8-1 8-2
MSC.visualNastran Desktop FEA Exercise Workbook. Foot Support
MSC.visualNastran Desktop FEA Exercise Workbook Foot Support WS3.1-2 Objectives This exercise is design to introduce vibration analysis in visualnastran Desktop. You will determine the natural frequencies
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
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
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.
POST-PROCESSING A RATCHET WHEEL
A POST-PROCESS CASE STUDY POST-PROCESSING A RATCHET WHEEL The objective of this case study is to run a post process analysis of a steel ratchet wheel subjected to a set of forces. We will observe the stresses
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.
Case Study 2: Piezoelectric Circular Plate
Case Study 2: Piezoelectric Circular Plate PROBLEM - 3D Circular Plate, kp Mode, PZT4, D=50mm x h=1mm GOAL Evaluate the operation of a piezoelectric circular plate having electrodes in the top and bottom
A pipe bend is subjected to a concentrated force as shown: y All dimensions in inches. Material is stainless steel.
Problem description A pipe bend is subjected to a concentrated force as shown: y 15 12 P 9 Displacement gauge Cross-section: 0.432 18 x 6.625 All dimensions in inches. Material is stainless steel. E =
Engineering 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
SDC. 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
Engineering 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
Start AxisVM by double-clicking the AxisVM icon in the AxisVM folder, found on the Desktop, or in the Start, Programs Menu.
4. MEMBRANE MODEL 1.1. Preprocessing with surface elements Start New Start AxisVM by double-clicking the AxisVM icon in the AxisVM folder, found on the Desktop, or in the Start, Programs Menu. Create a
Exercise 1: Axle Structural Static Analysis
Exercise 1: Axle Structural Static Analysis The purpose of this exercise is to cover the basic functionality of the Mechanical Toolbar (MTB) in the context of performing an actual analysis. Details of
Engineering 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
Post-Processing of Time-Dependent Results
LESSON 21 Post-Processing of Time-Dependent Results 49.26 47.23 45.19 18.70 43.15 41.11 39.07 37.04 35.00 32.96 30.92 49.26 28.89 26.85 24.81 Y Z X Objectives: 22.77 20.73 18.70 default_fringe : Max 49.26
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 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...
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
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.