![APPENDIX B Cantilever Beam (Sol 101)
2. Create a curve to define a geometrical representation of the beam.
xGeometry
Action: Create
Object: Curve
Method: XYZ
u Auto Execute
Vector Coordinates List: < 5, 0, 0 >
Origin Coordinates List: [0, 0, 0]
Apply
3. Discretize the geometry model with BAR2 elements. The element
length is determined by the Global Edge Length parameter.
x Finite Elements
Action: Create
Object: Mesh
Type: Curve
Global Edge Length: 0.5
Element Topology: Bar2
Curve List: Curve 1
Apply
Show all entity labels by selecting the Show Labels icon on the Top
Menu Bar
Show Labels
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-5](https://image.slidesharecdn.com/appendixbfinal-120609102520-phpapp02/85/Appendix-b-final-5-320.jpg)
![APPENDIX B Cantilever Beam (Sol 101)
Apply
The Current Constitutive Models form should appear as below:
Linear Elastic - [,,,,] - [Active]
Cancel
5. Define the properties of your beam model using the specified
section properties data. Here is where the material defined in the
previous operation is referenced. Be sure to specify the XY-
orientation vector correctly. Also, remember to specify the
stress recovery coefficients correctly. Otherwise, it will be
impossible to recover bending stresses.
x Properties
Action: Create
Object: 1D
Method: Beam
Property Set Name: bar
Input Properties...
Material Name: m:mat_1
Bar Orientation: < 0., 1., 0. >
Now, activate the Beam Library by clicking the icon shown below
Beam Library (Create Section)
Create
Standard Shapes
New Section Name: sect_1
MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-7](https://image.slidesharecdn.com/appendixbfinal-120609102520-phpapp02/85/Appendix-b-final-7-320.jpg)
Appendix b final
- 1. APPENDIX B Linear Static Analysis of a Cantilever Beam Using Beam Library (SI Units) Objectives: s Create a geometrical representation of a cantilever beam. s Use the geometry model to define an MSC/NASTRAN analysis model comprised of CBAR elements. s Prepare an MSC/NASTRAN input file for a linear static analysis. s Visualize analysis results. MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 2. B-2 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 3. APPENDIX B Cantilever Beam (Sol 101) Model Description: Below is a finite element representation of the beam structure shown on page 7-1. The beam has a hollow, rectangular cross-section as shown below in View A-A. The wall thickness is constant. The span of the beam is 5 m and has a fixed boundary condition at X = 0 and a tip force of 1000 N is applied at X = 5 m in the negative Y-direction. The beam undergoes pure bending as a result of this applied load. Y 1000.0 Z X A 1 2 3 4 5 6 7 8 9 10 123456 A Ye D b C 0.01 a a Ze 0.2 View A-A E b F 0.1 Elastic Modulus: 7.1e10 N/m2 Poisson Ratio: 0.3 Density: 2.704e3 kg/m3 Area: 5.600e-3 m2 Iaa( I1-1): 2.780e-5 m4 Ibb( I2-2): 8.990e-6 m4 J: 2.090e-5 m4 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-3
- 4. Suggested Exercise Steps: s Open a new database. s Create a curve and mesh it with bar elements (CBAR). Use the meshing feature so that elements and nodes (GRID) will be generated automatically by MSC/PATRAN. s Define material (MAT1) and element (PBAR) properties. s Verify XY-orientation vectors for bar elements. s Apply a fixed boundary constraint (SPC1) at one end of the beam and a transverse force to the free end of the beam (FORCE). s Use the load and boundary condition sets to define a loadcase (SUBCASE). s Prepare the model for a Linear Static analysis (SOL 101 and PARAMs). s Generate and submit input file to the MSC/NASTRAN solver. s Post-process results. s Quit MSC/PATRAN. Exercise Procedure: 1. Create a new database called cantilever_beam.db. File/New... New Database Name: cantilever_beam OK In the New Model Preference form set the following: Tolerance: x Default Analysis Code: MSC/NASTRAN Analysis Type: Structural OK B-4 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 5. APPENDIX B Cantilever Beam (Sol 101) 2. Create a curve to define a geometrical representation of the beam. xGeometry Action: Create Object: Curve Method: XYZ u Auto Execute Vector Coordinates List: < 5, 0, 0 > Origin Coordinates List: [0, 0, 0] Apply 3. Discretize the geometry model with BAR2 elements. The element length is determined by the Global Edge Length parameter. x Finite Elements Action: Create Object: Mesh Type: Curve Global Edge Length: 0.5 Element Topology: Bar2 Curve List: Curve 1 Apply Show all entity labels by selecting the Show Labels icon on the Top Menu Bar Show Labels MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-5
- 6. The completed model should appear as follows: 1 1 2 2 3 3 4 4 5 5 6 1 6 7 7 8 8 9 9 10 10 11 2 Y Z X 4. Define a material using the specified modulus of elasticity, Poisson ratio and density. x Materials Action: Create Object: Isotropic Method: Manual Input Material Name: mat_1 Input Properties... Constitutive Model: Linear Elastic Elastic Modulus = 7.10e10 Poisson Ratio = 0.3 Density = 2.65e4 B-6 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 7. APPENDIX B Cantilever Beam (Sol 101) Apply The Current Constitutive Models form should appear as below: Linear Elastic - [,,,,] - [Active] Cancel 5. Define the properties of your beam model using the specified section properties data. Here is where the material defined in the previous operation is referenced. Be sure to specify the XY- orientation vector correctly. Also, remember to specify the stress recovery coefficients correctly. Otherwise, it will be impossible to recover bending stresses. x Properties Action: Create Object: 1D Method: Beam Property Set Name: bar Input Properties... Material Name: m:mat_1 Bar Orientation: < 0., 1., 0. > Now, activate the Beam Library by clicking the icon shown below Beam Library (Create Section) Create Standard Shapes New Section Name: sect_1 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-7
- 8. Click on the icon shown below to access the Box Section menu. Box Section The menu should appear in the right half of the window. Enter the following dimensions into it. W= 0.1 H= 0.2 t1 = 0.01 t2 = 0.01 Calculate/Display The window shown below should appear. B-8 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 9. APPENDIX B Cantilever Beam (Sol 101) OK OK Select Members: Curve 1 Add Apply 6. 7. Graphically assess the orientation vectors that are required on the CBAR entries in the MSC/NASTRAN input file. These vectors define the local XY-plane for each bar element. Since the element property created was applied to the geometry model instead of the analysis model, graphical display of respective attributes will appear on the geometry model by default. To display attributes such as the orientation vectors on our analysis model, we must change an option in Display/Load/BC/Elem. Props... The node labels may be deactivated for clarity. Display/Load/BC/Elem. Props... s Show on FEM Only Beam Display: 3D: Full-Span+Offsets Apply Cancel Change the action in the Element Properties form to Show. Action: Show Existing Properties: Definition of XY Plane Display Method: Vector Plot Select Group: default_group Apply MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-9
- 10. The display should appear as follows: 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1.000 1 1 2 2 3 3 4 4 5 5 1 6 6 7 7 8 8 9 9 10 10 2 11 Y Z X 8. Reset the Functional Assignment Display back to geometry. Display/Load/BC/Elem. Props... u Show on FEM Only Apply Cancel 8a. Define the cantilever boundary condition by creating displacement constraints and applying them to the geometry model. x Loads/BCs Action: Create Object: Displacement Type: Nodal B-10 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 11. APPENDIX B Cantilever Beam (Sol 101) New Set Name: fixed Input Data... Translation < T1 T2 T3 > < 0, 0, 0 > Rotation <R1 R2 R3> < 0, 0, 0 > OK Select Application Region... Geometry Filter: x Geometry Select Geometric Entities: Point 1 Add OK Apply 9. The tip force which causes the beam to bend is defined as follows: x Loads/BCs Action: Create Object: Force Type: Nodal New Set Name: y_load Input Data... Force <F1 F2 F3> < , -1000, > OK Select Application Region... Geometry Filter: x Geometry Select Geometric Entities: Point 2 Add OK MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-11
- 12. Apply Refresh the display by selecting the brush icon on the Top Menu Bar. Refresh Graphics Create a load case which references the forces and boundary conditions that have been defined. x Load Cases Action: Create Load Case Name: sub_1 Load Case Type: Static Assign/Prioritize Loads/BCs (Click each selection until all Displ_fixed Loads/BCs have one entry in the spreadsheet)* Force_y_load * REMINDER: Make sure that the LBC Scale Factor column shows the proper value for each entry. OK Apply 10. For clarity, create a new group called fem_only. This group will contain only analysis model entities. Group/Create... New Group Name: fem_only s Make Current s Unpost All Other Groups Group Contents: Add All FEM Apply Cancel B-12 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 13. APPENDIX B Cantilever Beam (Sol 101) 11. Again, for clarity, shrink the elements by 10%; this allows us to easily assess the element connectivities. Use the Display/Finite Elements... option. Display/Finite Elements... FEM Shrink: 0.10 Apply Cancel 12. To display the load and boundary conditions on the analysis model, change the action in the Loads/BCs form to Plot Markers. 12a. Recall that because the loads and boundary conditions you defined were applied to the geometry model, the Functional Assignment Display must be set to FEM. Display/Load/BC/Elem. Props... s Show on FEM Only Apply Cancel 12b. Plot the load and boundary condition markers. x Loads/BCs Action: Plot Markers Select all sets in the Assigned Load/BC Sets box by highlighting them. Apply to the current group fem_only. Assigned Load/BCs Sets: Displ_fixed Force_y_load Select Groups: fem_only Apply When you are done, you will see the load and boundary conditions MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-13
- 14. displayed as follows:: 1000. 1123456 1 2 2 3 3 4 4 5 5 6 6 7 7 8 8 9 9 10 10 11 Y Z X Reset the display by selecting the broom icon on the Top Menu Bar. Reset Graphics 13. You are now ready to generate an input file for analysis. Click on the Analysis radio button on the Top Menu Bar and complete the entries as shown below. x Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: cantilever_beam Translation Parameters... B-14 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 15. APPENDIX B Cantilever Beam (Sol 101) OUTPUT2 Format: Binary MSC/NASTRAN Version: ??? set to current version 70 OK Solution Type... Solution Type: x Linear Static Solution Parameters... s Database Run s Automatic Constraints Data Deck Echo: Sorted Wt.- Mass Conversion = 1.000 (for SI units) OK OK Subcase Select... Subcases For Solution sub_1 Sequence: Subcases Selected: Default (click to deselect) OK Apply An input file named cantilever_beam.bdf will be generated. This process of translating your model into an input file is called the Forward Translation. The Forward Translation is complete when the Heartbeat turns green. 14. If all is well, you can submit the input file to MSC/NASTRAN for analysis. To do this, find an available xterm window and at the prompt enter: nastran cantilever_beam.bdf scr=yes Monitor the run using the UNIX ps command. MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-15
- 16. 14a. When the run is completed, edit the cantilever_beam.f06 file and search for the word FATAL. If none exists, search for the word WARNING. Determine whether or not existing WARNING messages indicate modeling errors. 14b. While still editing cantilever_beam.f06, search for the word D I S P L A C E (spaces are necessary) What is the y-component of the tip deflection vector? disp Y = What is the %error of this deflection versus the theoretical tip deflection? %error = Search for the word: S T R E S S (spaces are necessary) What is the maximum positive stress due to bending? max. stress = What is the %error of this stress versus the theoretical maximum positive bending stress? %error = 15. Proceed with the Reverse Translation process, that is, importing the cantilever_beam.op2 results file into MSC/PATRAN. To do this, return to the Analysis form and proceed as follows: x Analysis Action: Read Output2 Object: Result Entities Method: Translate Select Results File... B-16 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)
- 17. APPENDIX B Cantilever Beam (Sol 101) Filter Selected Results File: select the desired .op2 file OK Apply When translation is completed and the Heartbeat turns green, bring up the Results form. x Results Action: Create Object: Quick Plot Choose the desired result case in the Select Result Cases list and select the result(s) in the Select Fringe Result list and/or in the Select Deformation Result list. And hit Apply to view the result(s) in the viewport. If you wish to reset your display graphics to the state it was in before you began post-processing your model, remember to select the broom icon. Reset Graphics Quit MSC/PATRAN when you have completed this exercise. MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5) B-17
- 18. B-18 MSC/NASTRAN 120 Exercise Workbook - Version 70 (MSC/PATRAN 7.5)