The Essence of Result Post- Processing
|
|
- Edwin Wood
- 6 years ago
- Views:
Transcription
1 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 properties. symmetric boundary constraints. edge pressure to model. Run the analysis and read the results back into MSC.Patran. Generate a fringe plot of X stress tensor and compare results. MSC.Nastran 120 Exercise Workbook E-1
2 E-2 MSC.Nastran 120 Exercise Workbook
3 APPENDIX E The Essence of Result Post-Processing Model Description: Figure E.1 is a schematic of a plate with a circular hole at the center. The dimensions and loads are indicated. The finite element model will be simplified by creating the 1/4 tension coupon model with two simple surfaces as shown in Figure E.2. The plate is inches thick; therefore it will be modeled with shell elements. The tension coupon will have the properties of Table E.1. The resulting finite element model will have X- and Y-symmetry constraints with an additional constraint for translation in the Z-direction. The uniform edge pressure load of 100 psi will be applied to the right edge. Since the Patran edge pressure convention is in terms of lb/in, 100 psi must be converted to a running load by multiplying the pressure by the thickness of the plate. Figure E.1 - Plate with Circular Hole psi psi Y Z X 10. Table E.1 - Tension Coupon Properties Elastic Modulus: 10E+06 psi Poisson Ratio 0.3 Plate Thickness: in Figure E.2 - Simplified Model with Dimensions Y Z X 5. MSC.Nastran 120 Exercise Workbook E-3
4 Suggested Exercise Steps: Create the necessary curves and surfaces of the tension coupon geometry and mesh the geometry to create a finite element model. Define symmetric boundary constraints and apply a uniform pressure to one edge (TENSION_LOAD). Define material (MAT_1) and element properties (PSHELL). Prepare the model for a Linear Static Analysis. Generate and submit an input file to MSC.Nastran. Generate a fringe plot of σ xx. Review the results. E-4 MSC.Nastran 120 Exercise Workbook
5 APPENDIX E The Essence of Result Post-Processing Exercise Procedure: 1. Open a new database called appendix_e.db. File/New... New Database Name appendix_e OK In the New Model Preference form set the following: Tolerance Analysis code: OK Default MSC/NASTRAN Create the necessary geometry for the plate model. NOTE: Whenever possible, toggle off the Auto Execute option by left clicking the check box. 2. Construct circular arcs to represent the outline of the model. Because the mapped surfaces in MSC.Patran can have up to 4 edges, the arc will be created in 2 steps. Geometry Object: Method: Radius 1.0 Start Angle 0.0 End Angle 45.0 Radius 1.0 Start Angle 45.0 End Angle 90.0 Create Curve 2D ArcAngles MSC.Nastran 120 Exercise Workbook E-5
6 3. Referring to the model dimensions (see Figure E.2), the outer edges of the geometry are created through the following steps: First the top right. Geometry Object: Method: To create the top edge: 4. Create two surfaces using the curves made in the previous steps. Figure E.3 - Surface and Curve Locations Create Curve XYZ Vector Coordinates List < 0, 2, 0 > Origin Coordinates List [5, 0, 0] Vector Coordinates List < -5, 0, 0 > Origin Coordinates List [5, 2, 0] Curve 4 Surface 2 Curve 3 Curve 2 Surface 1 Curve 1 E-6 MSC.Nastran 120 Exercise Workbook
7 APPENDIX E The Essence of Result Post-Processing Geometry Object: Method: Complete the surface model. 5. Create a Finite Element Model by meshing the surface. It is essential to know the direction of each of the curves and lines. The direction will determine the bias ratio (L2/L1) of the mesh seeds. In steps 2 to 4, the geometry of this model was created so that the direction of the lines, curves and surfaces coincide with Figure E.4. Simply following the next step will indicate the curves and lines directions. Figure E.4 Create Surface Curve Starting Curve List: Curve 1 Ending Curve List: Curve 3 Starting Curve List: Curve 2 Ending Curve List: Curve a) Curve and Line Directions b) Mesh Seeds and Bias Ratio 6 elem 1:4 3 elem 1:1 6 elem 4:1 MSC.Nastran 120 Exercise Workbook E-7
8 First the elements with mesh seed ratios. Finite Elements Object: Type: Create Mesh Seed One Way Bias Num Elems and L2/L1 Number= 6 L2/L1= 4 Curve List Surface 1.1 Change the bias ratio (L2/L1). Number= 6 L2/L1= 0.25 Curve List Curve 2 Finally, the uniform mesh seed. Finite Elements (Select the bottom edge) (Select the top half of arc) Object: Type: Create Mesh Seed Uniform Num Elems and L2/L1 Number= 3 Curve List Curve 1 (Select the bottom half of arc) E-8 MSC.Nastran 120 Exercise Workbook
9 APPENDIX E The Essence of Result Post-Processing Mesh the surface. Finite Elements Create Object: Mesh Type: Surface Isomesh Surface List Surface 1, 2 Before continuing, equivalence the entire model to delete any duplicate nodes created when meshing. Finite Elements Object: Type: Equivalence All Tolerance Cube The model should appear as below. Figure E.5 - Completed Model with Finite Element Mesh. MSC.Nastran 120 Exercise Workbook E-9
10 6. Create material properties for the plate. Materials Create Object: Isotropic Method: Manual Input Material Name mat_1 Input Properties... Elastic Modulus= 10E6 Poisson Ratio= 0.3 OK 7. Define element properties. Properties Create Dimension: 2D Type: Shell Property Set Name plate Input Properties... Material Name m:mat_1 Thickness OK Select Members Surface 1, 2 Add 8. the boundary conditions to the model using Loads/BCs. This model will have three different contraints sets. E-10 MSC.Nastran 120 Exercise Workbook
11 APPENDIX E The Essence of Result Post-Processing Figure E.6 - Boundary Condition Placement X-symmetry (constraint along edge) Tension-load (pressure along edge) Rigid_body (Point 1) Y-symmetry (constraint along edge) First, create the X-symmetry contraints placed on the left side of the model. Selecting geometry may be done by typing in entity id s or clicking them as shown in Figure E.6. Loads/BCs Object: Type: New Set Name Input Data... Create Displacement Nodal x_symmetry Translations <T1 T2 T3> < 0,, > Rotations <R1 R2 R3> <, 0, 0 > OK Select Application Region... Geometry Filter Geometry MSC.Nastran 120 Exercise Workbook E-11
12 The surface edge may be typed into the input box or by clicking on the edge itself. This is done by first choosing the Curve or Edge icon from the Select Menu. Curve or Edge Select Geometry Entities Surface 2.3 Add OK Next, create the Y-symmetry constraints. (see Figure E.6) New Set Name y_symmetry Input Data... Translations <T1 T2 T3> <, 0, > Rotations <R1 R2 R3> < 0,, 0 > OK Select Application Region... Geometry Filter Geometry Select Geometry Entities Surface 1.1 Add OK (see Fig. E.6) Finally, assign one extra constraint set to remove rigid body motion in Z-direction. New Set Name rigid_body Input Data... Translations <T1 T2 T3> <,, 0 > Rotations <R1 R2 R3> <,, > E-12 MSC.Nastran 120 Exercise Workbook
13 APPENDIX E The Essence of Result Post-Processing OK Select Application Region... Geometry Filter Geometry The point may be typed into the input box or by clicking on the edge itself. This is done by first choosing the Point or Vertex icon from the Select Menu. Point or Vertex Select Geometry Entities Point 1 (see Figure E.6) Add OK Now the pressure load may be added to the model. Loads/BCs Object: Type: New Set Name Target Element Type: Create Pressure Element Uniform tension_load 2D Input Data... Edge Pressure OK Select Application Region... Geometry Filter Geometry MSC.Nastran 120 Exercise Workbook E-13
14 Type in the selected edge in the input box or click on the right edge of the model. Use the Edge icon from the Select Menu. Edge Select 2D Elements or Edge Surface 1.2 Add OK (see Figure E.6) NOTE: Positive pressure is always going into the surface/edge according to MSC.Patran convention. Therefore, the tensile load must be applied as The finished model should resemble Figure E.7. Figure E.7: Finished Model and Critical Elements Element 24 Element 23 Element 22 Element Use the Reset Graphics and Refresh Graphics icons to clean up the display. Reset Graphics Refresh Graphics E-14 MSC.Nastran 120 Exercise Workbook
15 APPENDIX E The Essence of Result Post-Processing 9. Submit the model for analysis. Analysis Analyze Object: Entire Model Method: Analysis Deck Job Name Solution Type... Solution Type: OK appendix_e LINEAR STATIC An MSC.Nastran input file called appendix_e.bdf will be generated. This process of translating the model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC.Nastran 120 Exercise Workbook E-15
16 Submitting the Input File for Analysis: 10. Submit the input file to MSC.Nastran for analysis. 10a. To submit the MSC.Patran.bdf file for analysis, find an available UNIX shell window. At the command prompt enter: nastran appendix_e.bdf scr=yes. Monitor the run using the UNIX ps command. 11. When the run is completed, edit the appendix_e.f06 file and search for the word FATAL. If no matches exist, search for the word WARNING. Determine whether existing WARNING messages indicate modeling errors. E-16 MSC.Nastran 120 Exercise Workbook
17 APPENDIX E The Essence of Result Post-Processing Comparison of Results: 12. Compare the results obtained in the.f06 file with the results on the following pages. MSC.Nastran 120 Exercise Workbook E-17
18 Table E.2 - Stress Values of Critical Elements in Tension Coupon S T R E S S E S I N Q U A D R I L A T E R A L E L E M E N T S ( Q U A D 4 ) OPTION = BILIN ELEMENT FIBRE STRESSES IN ELEMENT COORD SYSTEM PRINCIPAL STRESSES (ZERO SHEAR) ID GRID-ID DISTANCE NORMAL-X NORMAL-Y SHEAR-XY ANGLE MAJOR MINOR VON MISES 21 CEN/ E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E CEN/ E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E CEN/ E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E CEN/ E E E E E E E E E E E E E E E E E E E E E+02 ELEMENT FIBRE STRESSES IN ELEMENT COORD SYSTEM PRINCIPAL STRESSES (ZERO SHEAR) ID GRID-ID DISTANCE NORMAL-X NORMAL-Y SHEAR-XY ANGLE MAJOR MINOR VON MISES E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E+02 E-18 MSC.Nastran 120 Exercise Workbook
19 APPENDIX E The Essence of Result Post-Processing 13. MSC.Nastran Users have finished this exercise. MSC.Patran Users should proceed to the next step. 14. Proceed with the Reverse Translation process, that is attaching the appendix_e.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Object: Method: Select Results File... Select Results File Attach XDB Result Entities Local appendix_e.xdb When the translation is complete bring up the Results form. 15. Post process the results. Generate the fringe plot of the X stress tensor. Results Object: Create Fringe Choose the Select Results icon. Select Results Select Result Case(s) Select Fringe Result Position...(At Z1) Close Quantity: Default, Static Subcase Stress Tensor X Component MSC.Nastran 120 Exercise Workbook E-19
20 Click on the Target Entities icon. Target Entities Target Entity: Current Viewport NOTE: This feature allows controls which elements the stresses will be plotted on. Click on the Display Attributes icon. Display Attributes Style: Display: Title: Discrete/Smooth Free Edges Tension Coupon, Stress Tensor, - X Component, At Z1 Go to the Plot Options menu. Plot Options Coordinate Transformation: None Filter Values: Domain: Method: Extrapolation: None All Entities Derive/Average Shape Fn. The display should resemble Figure E.8. E-20 MSC.Nastran 120 Exercise Workbook
21 APPENDIX E The Essence of Result Post-Processing Figure E Examine the results. Question 1: What coordinate is the XX in reference to? Is it referring to global, element, material,...? Question 2: Does the plot match the Nastran results listed in Table E.2? 17. Create a different fringe plot and review the results. Click on the Plot Options icon. Plot Options Define the XX axis in the global coordinate system. Coordinate Transformation: Global Filter Values: None Turn off nodal averaging since Nastran results are reported at each element. Domain: Method: Extrapolation: None Derive/Average Shape Fn. MSC.Nastran 120 Exercise Workbook E-21
22 The plot should resemble Figure E.9. Figure E.9 The new results are significantly different from the previous plot. However, this plot correctly illustrates the individual element stresses in global X-axis. Question: Does this plot match the results listed in Table E.2? Why not? 18. Create another fringe plot and review the results. Click on the Plot Options icon. Plot Options This time define the XX axis by changing the previous global coordinate system to none. Coordinate Transformation: None Filter Values: None E-22 MSC.Nastran 120 Exercise Workbook
23 APPENDIX E The Essence of Result Post-Processing Turn off the averaging domain since Nastran results are reported at each element. Domain: Method: Extrapolation: None Derive/Average Shape Fn. The plot should resemble Figure E.10. Figure E.10 Cross reference this plot with the previous results table. Be certain that they are the same. In the interest of further study, the following is a continuation of this exercise in order to examine differences in analysis result values. 19. Create a new coordinate system. Geometry Object: Method: Create Coord 3Point Origin [0, 0, 0] MSC.Nastran 120 Exercise Workbook E-23
24 Point on Axis 3 [0, 0, 1] Point on Plane 1-3 [1, 1, 0] Generate the X stress plot again, but use CID option. Results Object: Create Fringe Click on the Select Results icon. Select Results Select Result Case(s) Select Fringe Result Position...(At Z1) Close Quantity: Default, Static Subcase Stress Tensor X Component The previous form selections are still valid and will not be changed, therefore, skip the Target Entities and Display Attributes icons and continue on to the Plot Options form. Click on the Plot Options icon. Plot Options Coordinate Transformation: CID Select Coordinate Frame Coord 1 Filter Values: None Domain: None Method: Derive/Average Extrapolation: Shape Fn. E-24 MSC.Nastran 120 Exercise Workbook
25 APPENDIX E The Essence of Result Post-Processing See Fig. E.11 and review results. Figure E.11 Quit MSC.Patran after finishing this exercise. MSC.Nastran 120 Exercise Workbook E-25
26 E-26 MSC.Nastran 120 Exercise Workbook
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
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 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 informationLinear 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
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 informationElastic 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
More informationModal Analysis of a Beam (SI Units)
APPENDIX 1a Modal Analysis of a Beam (SI Units) Objectives Perform normal modes analysis of a cantilever beam. Submit the file for analysis in MSC.Nastran. Find the first three natural frequencies and
More informationModal 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.
More informationAlternate Bar Orientations
APPENDIX N Alternate Bar Orientations Objectives: The effects of alternate bar orientation vector. MSC.Nastran 120 Exercise Workbook N-1 N-2 MSC.Nastran 120 Exercise Workbook APPENDIX N Alternate Bar Orientations
More informationLoad 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
More informationRestarting 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
More informationRigid 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
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 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 informationAPPENDIX 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...
More informationNonlinear 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.
More informationShear 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
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 informationPost-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
More informationModal 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
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 informationLinear 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
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 informationLinear Buckling Load Analysis (without spring)
WORKSHOP PROBLEM 4a Linear Buckling Load Analysis (without spring) Objectives: Demonstrate the use of linear buckling analysis. MSC/NASTRAN 103 Exercise Workbook 4a-1 4a-2 MSC/NASTRAN 103 Exercise Workbook
More informationWORKSHOP 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.
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 informationElasto-Plastic Deformation of a Truss Structure
WORKSHOP PROBLEM 8 Elasto-Plastic Deformation of a Truss Structure Objectives: Demonstrate the use of elasto-plastic material properties. Create an enforced displacement on the model. Create an XY plot
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 informationTransient 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
More informationPost-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:
More informationSpatial 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
More informationNormal Modes with Differential Stiffness
WORKSHOP PROBLEM 14b Normal Modes with Differential Stiffness Objectives Analyze a stiffened beam for normal modes. Produce an MSC/ NASTRAN input file that represent beam and load. Submit for analysis.
More informationLinear 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
More informationModal 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. Produce a MSC/NASTRAN input
More informationCylinder 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
More informationSpatial 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
More informationMSC/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
More informationPost 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
More informationNormal Modes Analysis of a Simply-Supported Stiffened Plate
APPENDIX C Normal Modes Analysis of a Simply-Supported Stiffened Plate Objectives: Manually convert a Linear Static analysis (Sol 101) input file to a Normal Modes analysis (Sol 103) input file. Learn
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 informationLinear and Nonlinear Analysis of a Cantilever Beam
LESSON 1 Linear and Nonlinear Analysis of a Cantilever Beam P L Objectives: Create a beam database to be used for the specified subsequent exercises. Compare small vs. large displacement analysis. Linear
More informationUsing 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
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 informationPost 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
More informationDirect Transient Response Analysis
WORKSHOP PROBLEM 3 Direct Transient Response Analysis Objectives Define time-varying excitation. Produce a MSC/NASTRAN input file from dynamic math model created in Workshop 1. Submit the file for analysis
More informationLoad 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
More informationProjected 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
More informationAnalysis 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
More informationDirect Transient Response Analysis
WORKSHOP 3 Direct Transient Response Analysis Objectives Define time-varying excitation. Produce a MSC.Nastran input file from dynamic math model created in Workshop 1. Submit the file for analysis in
More informationPost 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
More informationProjected 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
More informationEXERCISE 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:
More informationSpring Element with Nonlinear Analysis Parameters (Multi-Step Analysis)
WORKSHOP 32c Spring Element with Nonlinear Analysis Parameters (Multi-Step Analysis) Objectives: Demonstrate the effects of geometric nonlinear analysis in SOL 106 (nonlinear statics). incremental loads
More informationMaterials, Load Cases and LBC Assignment
LESSON 4 Materials, Load Cases and LBC Assignment 5.013 5.000 4.714 30000 4.429 4.143 3.858 3.572 3.287 3.001 2.716 2.430 2.145 1.859 20000 1.574 1.288 default_fringe : 1.003 Max 2.277 @Elm 40079.1 Min
More informationPost-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
More informationSpring Element with Nonlinear Analysis Parameters (filter using restart)
WORKSHOP PROBLEM 1e Spring Element with Nonlinear Analysis Parameters (filter using restart) Objectives: Demonstrate another use of the restart feature in a multistep analysis by keeping only the first
More informationLarge-Scale Deformation of a Hyperelastic Material
WORKSHOP PROBLEM 5 Large-Scale Deformation of a Hyperelastic Material Objectives: Demonstrate the use of hyperelastic material properties. Create an accurate deformation plot of the model. MSC/NASTRAN
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 informationMass 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
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 informationLinear 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
More informationModal Transient Response Analysis
WORKSHOP 4 Modal Transient Response Analysis Z Y X Objectives Define time-varying excitation. Produce a MSC.Nastran input file from a dynamic math model, created in Workshop 1. Submit the file for analysis
More informationModal Transient Response Analysis
WORKSHOP PROBLEM 4 Modal Transient Response Analysis Z Y X Objectives Define time-varying excitation. Produce a MSC/NASTRAN input file from a dynamic math model, created in Workshop 1. Submit the file
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 informationHeat 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
More informationPost 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
More informationANSYS AIM Tutorial Structural Analysis of a Plate with Hole
ANSYS AIM Tutorial Structural Analysis of a Plate with Hole Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Analytical vs. Numerical Approaches
More informationModal Transient Response Analysis
WORKSHOP 22 Modal Transient Response Analysis Z Y X Objectives Define time-varying excitation. Produce a MSC.Nastran input file from a dynamic math model, created in Workshop 1. Submit the file for analysis
More informationVerification and Property Assignment
LESSON 9 Verification and Property Assignment Objectives: Prepare the model for analysis by eliminating duplicate nodes and verifying element attributes. material and element properties. PATRAN 301 Exercise
More informationImporting 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
More informationLinear 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
More informationMerging Databases LESSON 2. Objectives: Construct two databases which have distinct similarities and differences.
LESSON 2 Merging Databases Objectives: Construct two databases which have distinct similarities and differences. See how PATRAN resolves model conflicts and differences when the two databases are imported
More informationPATRAN/ABAQUS PRACTICE
UNIVERSITY OF ILLINOIS AT URBANA-CHAMPAIGN College of Engineering CEE570/CSE551 Finite Element Methods (in Solid and Structural Mechanics) Spring Semester 2014 PATRAN/ABAQUS PRACTICE This handout provides
More informationFinite 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
More informationComposite 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
More informationThermal Analysis Using MSC.Nastran
MSC.Software Corporation 815 Colorado Boulevard Los Angeles, California 90041-1777 Tel: (323) 258-9111 Fax: (323) 259-3838 United States MSC.Patran Support Tel: 1-800-732-7284 Fax: 714-9792990 Tokyo, Japan
More informationRigid 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
More informationBuilding the Finite Element Model of a Space Satellite
LESSON 3 Building the Finite Element Model of a Space Satellite 30000 30001 Objectives: mesh & MPC s on a Space Satellite Perform Model and Element Verification. Learn how to create 0-D, 1-D and 2-D elements
More informationBuilding the Finite Element Model of a Space Satellite
Exercise 4 Building the Finite Element Model of a Space Satellite 30000 20000 Objectives: mesh & MPC s on a Space Satellite. Perform Model and Element Verification. Learn how to control mesh parameters
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 informationAbaqus CAE Tutorial 6: Contact Problem
ENGI 7706/7934: Finite Element Analysis Abaqus CAE Tutorial 6: Contact Problem Problem Description In this problem, a segment of an electrical contact switch (steel) is modeled by displacing the upper
More informationPost 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
More informationA 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 =
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 informationImporting 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
More informationAnalysis Steps 1. Start Abaqus and choose to create a new model database
Source: Online tutorials for ABAQUS Problem Description The two dimensional bridge structure, which consists of steel T sections (b=0.25, h=0.25, I=0.125, t f =t w =0.05), is simply supported at its lower
More informationCreating 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..
More informationImporting 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
More informationFinite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole
Problem Specification Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole Consider the classic example of a circular hole in a rectangular plate of constant thickness. The plate
More informationIn-plane principal stress output in DIANA
analys: linear static. class: large. constr: suppor. elemen: hx24l solid tp18l. load: edge elemen force node. materi: elasti isotro. option: direct. result: cauchy displa princi stress total. In-plane
More informationSimilar 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
More informationLinear 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
More informationChapter 2. Structural Tutorial
Chapter 2. Structural Tutorial Tutorials> Chapter 2. Structural Tutorial Static Analysis of a Corner Bracket Problem Specification Problem Description Build Geometry Define Materials Generate Mesh Apply
More informationNonlinear 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
More informationAbaqus/CAE Axisymmetric Tutorial (Version 2016)
Abaqus/CAE Axisymmetric Tutorial (Version 2016) Problem Description A round bar with tapered diameter has a total load of 1000 N applied to its top face. The bottom of the bar is completely fixed. Determine
More informationfile://c:\documents and Settings\sala\Configuración local\temp\~hha54f.htm
Página 1 de 26 Tutorials Chapter 2. Structural Tutorial 2.1. Static Analysis of a Corner Bracket 2.1.1. Problem Specification Applicable ANSYS Products: Level of Difficulty: Interactive Time Required:
More 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 informationSteady State Radiative Boundary Conditions
Exercise 22 Steady State Radiative Boundary Conditions Objectives: Create a 2D model that incorporates two enclosures. Define separate radiative boundary conditions for gray body and wave length dependent
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 information