![14a-10 MSC/NASTRAN 102 Exercise Workbook
Exercise Procedure:
1. Users who are not utilizing MSC/PATRAN for generating an input file
should go to Step 10, otherwise, proceed to step 2.
2. Create a new database named prob14a.db.
In the New Model Preference form set the following:
3. Activate the entity labels by selecting the Show Labels icon on the tool-
bar.
4. Create a curve.
File/New Database
New Database Name prob14a
OK
Tolerance ◆ Default
Analysis Code: MSC/NASTRAN
OK
◆ Geometry
Action: Create
Object: Curve
Method: XYZ
Vector Coordinates List <100, 0, 0>
Origin Coordinates List [ 0, 0, 0]
Apply
Show Labels](https://image.slidesharecdn.com/prob14a-241016154626-b0c8bebd/85/Modal-Analysis-of-a-Beam-using-Ansys-Tool-10-320.jpg)
Modal Analysis of a Beam using Ansys Tool
- 1. WORKSHOP PROBLEM 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-1 Objectives ■ Perform normal modes analysis of a cantilever beam. ■ Submit the file for analysis in MSC/NASTRAN. ■ Find the first three natural frequencies and mode shapes of the beam.
- 2. 14a-2 MSC/NASTRAN 102 Exercise Workbook
- 3. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-3 Model Description: The goal of this example is to find the first 3 modes of a beam pinned at both ends. Figure 14a.1 below is a finite element representation of the beam. One end is contrained in all translation and the other is free to move in the X. Both ends are held in the X-rotation. Figure 14a.1-Grid Coordinates and Element Connectivities
- 4. 14a-4 MSC/NASTRAN 102 Exercise Workbook Figure 14a.2-Beam Cross Section Table 14a.1 Length 100 in Height 2 in Width 1 in Thickness 0.100 in Area 0.38 in2 I1 0.229 in4 I2 0.017 in4 0.1 in 0.1 in 0.1 in 1.0 in 1.0 in 2.0 in
- 5. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-5 Hand Calculations * I of the strong axis is used since translational Z DOF has been constrained by the permanent constraint. From Theory Mode Kn fn 1 9.87 23.85 Hz 2 39.5 95.46 Hz 3 88.8 214.59 Hz fn Kn 2π ----- - EIg Wl4 --------- - 1 2 ⁄ = fn Kn 1 2π ----- - 10 6 ×10 0.229 ( ) 386.4 ( ) 0.38 ( ) 0.101 ( ) 100 ( )4 ------------------------------------------------------ - 1 2 ⁄ = fn Kn 2.417 ( ) =
- 6. 14a-6 MSC/NASTRAN 102 Exercise Workbook Suggested Exercise Steps ■ Explicitly generate a finite element representation of the beam structure. (i.e., the grids (GRID) and element connectivities (CBAR) should be defined manually.) ■ Define material (MAT1) and element (PBARL) properties. ■ Apply the fixed boundary constraints (SPC1). ■ Prepare the model for a normal modes analysis (SOL 103 and PARAMS). ■ PARAM, WTMASS, 0.00259 ■ PARAM, COUPMASS, 1 ■ EIGRL (To select Lanczos.) ■ Generate an input file and submit it to the MSC/NASTRAN solver for normal modes analysis. ■ Review the results, specifically the eigenvalues.
- 7. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-7 ID SEMINAR,PROB1 __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ __________________________________________ CEND __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ __________________________________________________________ BEGIN BULK
- 8. 14a-8 MSC/NASTRAN 102 Exercise Workbook 1 2 3 4 5 6 7 8 9 10
- 9. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-9 1 2 3 4 5 6 7 8 9 10 ENDDATA
- 10. 14a-10 MSC/NASTRAN 102 Exercise Workbook Exercise Procedure: 1. Users who are not utilizing MSC/PATRAN for generating an input file should go to Step 10, otherwise, proceed to step 2. 2. Create a new database named prob14a.db. In the New Model Preference form set the following: 3. Activate the entity labels by selecting the Show Labels icon on the tool- bar. 4. Create a curve. File/New Database New Database Name prob14a OK Tolerance ◆ Default Analysis Code: MSC/NASTRAN OK ◆ Geometry Action: Create Object: Curve Method: XYZ Vector Coordinates List <100, 0, 0> Origin Coordinates List [ 0, 0, 0] Apply Show Labels
- 11. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-11 5. Create the finite element model and mesh the surface. 6. Create nodal displacements. ◆ Finite Elements Action: Create Object: Mesh Type: Curve Global Edge Length 10 Curve List Curve 1 Apply ◆ Loads/BCs Action: Create Object: Displacement Type: Nodal New Set Name disp1 Input Data... Translations <T1 T2 T3> <0 0 0> Rotations <R1 R2 R3> <0 , , > OK Select Application Region... ■ Geometry Select Geometry Entities Point 1 Add OK Apply New Set Name disp2 Input Data... Translations <T1 T2 T3> < , 0 0>
- 12. 14a-12 MSC/NASTRAN 102 Exercise Workbook 7. Create a set of material properties for the bar. Rotations <R1 R2 R3> <0 , , > OK Select Application Region... Select Geometry Entities Point 2 Add OK Apply New Set Name permanent_constraint Input Data... Translations <T1 T2 T3> < , , 0> Rotations <R1 R2 R3> <0 , 0 , > OK Select Application Region... Select Geometry Entities Curve 1 Add OK Apply ◆ Materials Action: Create Object: Isotropic Method: Manual Input Material Name alum Input Properties... Elastic Modulus = 10.0E6 Poisson Ratio = .3 Density = .101
- 13. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-13 8. Define the bar properties. Apply Cancel ◆ Properties Action: Create Dimension: 1D Type: Beam Property Set Name bar Input Properties... Material Name (Select from Material Property Sets box) m:alum ■ Use Beam Section <Click on Beam Library> New Section Name ibeam H 2 W1 1 W2 1 t 0.1 t1 0.1 t2 0.1 OK Bar Orientation Coord 0.2 OK Select Members Curve 1 Add Apply
- 14. 14a-14 MSC/NASTRAN 102 Exercise Workbook 9. Now, you will generate the input file for analysis. An MSC/NASTRAN input file called prob14a.bdf will be generated. The process of translating your model into an input file is called Forward Translation. The Forward Translation is complete when the Heartbeat turns green. MSC/PATRAN Users should proceed to step 11. ◆ Analysis Action: Analyze Object: Entire Model Method Analysis Deck Job Name prob14a Solution Type... Solution Type: ◆ NORMAL MODES Solution Parameters ... <deselect Automatic Constraints> ❒ Automatic Constraints Mass Calculation: Coupled Data Deck Echo: None Wt. -Mass Conversion = .00259 OK OK Subcase Create... Available Subcases Default Subcase Parameters... Number of Desired Roots = 3 OK Apply Cancel <to close form> Apply
- 15. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-15 Generating an input file for MSC/NASTRAN Users: MSC/NASTRAN users can generate an input file using the data from Table 14a.1. The result should be similar to the output below. 10. MSC/NASTRAN Input File: prob14a.dat SOL 103 TIME 600 CEND TITLE = Normal Modes Example SUBCASE 1 METHOD = 1 SPC = 1 VECTOR=ALL BEGIN BULK PARAM,WTMASS,.00259 PARAM,COUPMASS,1 EIGRL 1 3 0 PBARL 1 1 I + A + A 2. 1. 1. .1 .1 .1 CBAR 1 1 1 2 0. 1. 0. CBAR 2 1 2 3 0. 1. 0. CBAR 3 1 3 4 0. 1. 0. CBAR 4 1 4 5 0. 1. 0. CBAR 5 1 5 6 0. 1. 0. CBAR 6 1 6 7 0. 1. 0. CBAR 7 1 7 8 0. 1. 0. CBAR 8 1 8 9 0. 1. 0. CBAR 9 1 9 10 0. 1. 0. CBAR 10 1 10 11 0. 1. 0. MAT1 1 1.+7 .3 .101 GRID 1 0. 0. 0. 345 GRID 2 10. 0. 0. 345 GRID 3 20. 0. 0. 345 GRID 4 30. 0. 0. 345 GRID 5 39.9999 0. 0. 345 GRID 6 49.9999 0. 0. 345 GRID 7 60. 0. 0. 345 GRID 8 70. 0. 0. 345 GRID 9 80. 0. 0. 345 GRID 10 90. 0. 0. 345 GRID 11 100. 0. 0. 345 SPC1 1 1234 1 SPC1 1 234 11 ENDDATA
- 16. 14a-16 MSC/NASTRAN 102 Exercise Workbook Submit the input file for analysis 11. Submit the input file to MSC/NASTRAN for analysis. 11a. To submit the MSC/PATRAN .bdf file for analysis, find an available UNIX shell window. At the command prompt enter: nastran prob14a.bdf scr=yes. Monitor the run using the UNIX ps command. 11b. To submit the MSC/NASTRAN .dat file for analysis, find an available UNIX shell window. At the command prompt enter: nastran prob14a scr=yes. Monitor the run using the UNIX ps command. 12. When the run is completed, edit the prob14a.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. 13. While still editing prob14a.f06, search for the word: E I G E N (spaces are necessary) What are the first three modes? 1st = __________Hz 2nd = __________Hz 3rd = __________Hz Comparison of Results 14. Compare the results obtained in the .f06 file with the results on the following page:
- 17. WORKSHOP 14a Modal Analysis of a Beam MSC/NASTRAN 102 Exercise Workbook 14a-17 R E A L E I G E N V A L U E S MODE EXTRACTION EIGENVALUE RADIANS CYCLES GENERALIZED GENERALIZED NO. ORDER MASS STIFFNESS 1 1 2.239398E+04 1.496462E+02 2.381693E+01 1.000000E+00 2.239398E+04 2 2 3.549898E+05 5.958102E+02 9.482614E+01 1.000000E+00 3.549898E+05 3 3 1.771818E+06 1.331096E+03 2.118506E+02 1.000000E+00 1.771818E+06
- 18. 14a-18 MSC/NASTRAN 102 Exercise Workbook MSC/NASTRAN Users have finished this exercise. MSC/PATRAN Users should proceed to the next step. 15. Proceed with the Reverse Translation process, that is importing the prob14a.op2 results file into MSC/PATRAN. To do this, return to the Analysis form and proceed as follows: When the translation is complete bring up the Results form. To reset the graphics, click on this icon: You can go back and select any Results Case, Fringe Results or Deformation Results you are interested in. Quit MSC/PATRAN when you are finished with this exercise. ◆ Analysis Action: Read Output2 Object: Result Entities Method Translate Select Results File... Select Results File prob14a.op2 OK Apply ◆ Results Form Type: Basic Select Results Cases 1.1-Default, Mode 1:Freq=23.816 Select Deformation Result 1.1 Eigenvectors, Translational Apply Reset Graphics