Load Analysis of a Beam (using a point force and moment)

Transcription

1 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 applied on the tip. Prepare an MSC.Nastran input file for a linear static analysis. Review analysis results. Recover element forces. MSC.Nastran 105 Exercise Workbook 13a-1

2 13a-2 MSC.Nastran 105 Exercise Workbook

3 WORKSHOP 13a Load Analysis of a Beam Model Description: Part A (Beam w/ force and moment) Figure 13a-1 is a finite element representation of the beam shown on the exercise title page. The material properties for the model are specified in Table 13a.1. The beam cross section dimensions are specified in Table 13a.2. Since the applied load does not act on the center of the beam cross-section, a bending moment will be induced. One way to account for this effect is to use 3D solid elements to model the beam. However, because the geometry is well suited for a beam model, this is not a desirable solution. Another possibility is to decompose the load into an equivalent load at the centroid of the beam x-section and add apply a moment to the model. Figure 13a.2 illustrates the loads and boundary conditions for the model. Figure 13a.1 - Grid Coordinates and Element Connectivities [0, 0, 0] [10, 0, 0] [20, 0, 0] [30, 0, 0] [40, 0, 0] [50, 0, 0] Y Z X Figure 13a.2 - Loads and Boundary Conditions Y Z X MSC.Nastran 105 Exercise Workbook 13a-3

4 Table 13a.1 - Material Properties Elastic Modulus = 10E6 lb/in 2 Poisson s Ratio = 0.3 Table 13a.2 - Element Properties Beam Dimensions H W1 W2 t t1 t2 4.0 in. 2.0 in. 2.0 in. 0.1 in in in. Hand Calculation: Applied Moments M 3 = r f = = 2( in) 100( lb) 200( in lb) 13a-4 MSC.Nastran 105 Exercise Workbook

5 WORKSHOP 13a Load Analysis of a Beam Suggested Exercise Steps: Open a new database. Generate a finite element representation of the beam structure by meshing the curve with desired global edge length. Define material (MAT1) and element (PBAR) properties. fixed boundary constraints (SPC), a point force (FORCE), and a moment (MOMENT). Prepare the model for a linear static analysis (SOL 101 and PARAMs). Generate an input file and submit it to the MSC.Nastran solver. Post-process results. Review the results. MSC.Nastran 105 Exercise Workbook 13a-5

6 Exercise Procedure: 1. Users who are not utilizing MSC.Patran for generating an input file should go to Step 14 otherwise, proceed to Step Create a new database called lesson13a.db File/New New Database Name OK lesson13a In the New Model Preferences form set the following: Tolerance Analysis code: OK Default MSC/NASTRAN 1. Activate the entity labels by selecting the Show Labels button on the toolbar. Show Labels 1. Also, activate the Node Size button. Node Size 1. Create the parent geometry. Geometry Action: Create Object: Curve Method: XYZ Vector Coordinates List: <50, 0, 0 > Origin Coordinates List: [0, 0, 0] 13a-6 MSC.Nastran 105 Exercise Workbook

7 WORKSHOP 13a Load Analysis of a Beam 1. Mesh the parent geometry. Finite Elements Action: Create Object: Mesh Type: Curve Global Edge Length: 10 Element Topology: Bar2 Curve List: Curve 1 Figure 13a.3 - Nodal and Element Locations Y Z X 2. Next, define a material using the specified modulus of elasticity and Poisson s ratio. Materials Action: Create Object: Isotropic Method: Manual Input MSC.Nastran 105 Exercise Workbook 13a-7

8 Material Name: Input Properties... mat_1 Constitutive Model: Linear Elastic Elastic Modulus = 10e6 Poisson Ratio = 0.3 In the Current Constitutive Models data box, the line Linear Elastic - [,,,,] - [Active] appear. Click on Cancel to close the form. Cancel 3. Define element properties for the analysis model. Properties Action: Create Dimension: 1 D Type: Beam Property Set Name: Option(s): Input Properties... Material Name Click the beam library icon: beam General Section m:mat_1 Bar Orientation < 0, 1, 0 > Associate Beam Section Action: Create 13a-8 MSC.Nastran 105 Exercise Workbook

9 WORKSHOP 13a Load Analysis of a Beam Type: Standard Shape New Section Name: beam_section H 4.0 W1 2.0 W2 2.0 t 0.1 t t Calculate/Display Close OK OK Select Members: Elm 1:5 Add 4. Verify element connectivities. To make this step easier, use the element shrink option. Display/Finite Elements... FEM Shrink: Create constraints and apply them to the analysis model. Loads/BCs Action: Create Object: Displacement Type: Nodal MSC.Nastran 105 Exercise Workbook 13a-9

10 New Set Name: fixed Input Data... Translations < T1 T2 T3 > <0, 0, 0> Rotations < R1 R2 R3 > <0, 0, 0> OK Select Application Region... Geometry Filter: FEM Select Nodes: Node 1 Add OK Figure 13a.4 - Displacement Constraints Y Z X 13a-10 MSC.Nastran 105 Exercise Workbook

11 WORKSHOP 13a Load Analysis of a Beam 6. The beam element are modeled at the neutral axis of the actual 3-D beam. Since the axial load is offset from the neutral axis, there is an induced bending moment at the end of the beam. This bending moment is applied with the axial force below (See Hang Calculation). Loads/BCs Action: Create Object: Force Method: Nodal New Set Name: Input Data... load Force < F1 F2 F3 > < -100, 0, 0 > Moment < M1 M2 M3 > < 0, 0, 200 > OK Select Application Region... Geometry Filter: FEM Select Nodes: Node 6 Add OK To verify both the moment and the force, change the view to Isoview_1 by selecting this icon: Iso 1 View MSC.Nastran 105 Exercise Workbook 13a-11

12 Figure 13a.5 - The resultant forces will be displayed as follows: Y Z X 7. Next observe the beam in 3D to visualize where the force and moment are being applied. Display/Loads/BC/Elem. Props... Beam Display Cancel 3D: Full-Span + Offsets 13a-12 MSC.Nastran 105 Exercise Workbook

13 WORKSHOP 13a Load Analysis of a Beam Figure 13a.6-3D representation of the beam Y Z X 8. Generate an input file for analysis. Click on the Analysis radio button on the Top Menu Bar and complete the entries as shown here. Analysis Action: Analyze Object: Entire Model Method: Analysis Deck Job Name: lesson13a A MSC.Nastran input file called lesson13a.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.Patran Users should proceed to step 15. MSC.Nastran 105 Exercise Workbook 13a-13

14 Generating an input file for MSC.Nastran Users: 9. MSC.Nastran users can generate an input file using the data from 13a-3. The result should be similar to the output below (lesson13a.dat): ID SEMINAR, lesson13a SOL 101 TIME 600 CEND TITLE = MSC.Nastran job ECHO = NONE MAXLINES = SUBCASE 1 $ Subcase name : Default SUBTITLE=Default SPC = 2 LOAD = 2 DISPLACEMENT(SORT1,REAL)=ALL SPCFORCES(SORT1,REAL)=ALL STRESS(SORT1,REAL,VONMISES,BILIN)=ALL BEGIN BULK PARAM POST -1 PARAM PATVER 3. PARAM AUTOSPC YES PARAM INREL 0 PARAM ALTRED NO PARAM COUPMASS -1 PARAM K6ROT 0. PARAM WTMASS 1. PARAM,NOCOMPS,-1 PARAM PRTMAXIM YES $ Elements and Element Properties for region : beam PBAR A + A B + B CBAR CBAR CBAR CBAR CBAR $ Material Record : mat_1 MAT $ Nodes of the Entire Model GRID GRID GRID GRID GRID GRID a-14 MSC.Nastran 105 Exercise Workbook

15 WORKSHOP 13a Load Analysis of a Beam $ Loads for Load Case : Default SPCADD 2 1 LOAD $ Displacement Constraints of Load Set : fixed SPC $ Nodal Forces of Load Set : load FORCE $ Nodal Forces of Load Set : load MOMENT $ Referenced Coordinate Frames ENDDATA MSC.Nastran 105 Exercise Workbook 13a-15

16 SUBMITTING THE INPUT FILE FOR MSC.Nastran and MSC.Patran USERS: 10. Submit the input file to MSC.Nastran for analysis. 10a. To submit the MSC.Patran.bdf file, find an available UNIX shell window. At the command prompt enter nastran lesson13a.bdf scr=yes. Monitor the run using the UNIX ps command. 10b. To submit the MSC.Nastran.dat file, find an available UNIX shell window and at the command prompt enter nastran lesson13a scr=yes. Monitor the run using the UNIX ps command. 11. When the run is completed, edit the lesson13a.f06 file and search for the word FATAL. If no matches exist, search for the word WARN- ING. Determine whether existing WARNING messages indicate modeling errors. 11a. While still editing lesson13a.f06, search for the word: D I S P L A C E (spaces are necessary). 13a-16 MSC.Nastran 105 Exercise Workbook

17 MSC.Nastran 105 Exercise Workbook 13a-17 D I S P L A C E M E N T V E C T O R POINT ID. TYPE T1 T2 T3 R1 R2 R3 1 G G E E E-05 3 G E E E-04 4 G E E E-04 5 G E E E-04 6 G E E E-04 WORKSHOP 13a Load Analysis of a Beam

18 Comparison of Results: 12. Compare the results obtained in the.f06 file with the results on the previous page: Also compare the results in the.f06 file with the following hand calculations applicable to node #6. Deflection from the axial load: P L T1 = = A E 6 T1 = 5.15E 4 in 0.97 ( ) Deflection from the bending moment: M L 2 T = = I E 6 T2 = 9.43E 3 in 2 ( 2.65) ( ) Rotation at the end: M L R3 = = E I 6 R3 = 3.77E 4 rad ( ) ( 2.65) 13a-18 MSC.Nastran 105 Exercise Workbook

19 WORKSHOP 13a Load Analysis of a Beam 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, importing the lesson13a.xdb results file into MSC.Patran. To do this, return to the Analysis form and proceed as follows: Analysis Action: Attach XDB Object: Result Entities Method: Translate Select Results File... Selected Results File Ok lesson13a XDB You may reset the graphics if you click on this icon: Reset Graphics 15. When the translation is complete and the Heartbeat turns green, bring up the Results form. Find the deformation in the X-direction. Results Action: Create Object: Deformation Select Result Case(s) Select Deformation Result Show As: XX YY ZZ Default, Static Subcase Displacements, Translational Component MSC.Nastran 105 Exercise Workbook 13a-19

20 Figure 13a.7 - The Display Should Appear as Below: Note: Compare the results to what was found in the.f06 file on page 13a a. Find the deformation in the Y-direction. Results Action: Create Object: Deformation Select Result Case(s) Select Deformation Result Show As: XX YY ZZ Default, Static Subcase Displacements, Translational Component 13a-20 MSC.Nastran 105 Exercise Workbook

21 WORKSHOP 13a Load Analysis of a Beam Figure 13a.8 - The Display Should Appear as Below: Note: Compare the results to what was found in the.f06 file on page 13a b. Find the resultant deformation. Results Action: Create Object: Deformation Select Result Case(s) Select Deformation Result Show As: Default, Static Subcase Displacements, Translational Resultant MSC.Nastran 105 Exercise Workbook 13a-21

22 Figure 13a.9 - The Display Should Appear as Below: Note: Compare the results to what was found in the.f06 file on page 13a- 17. The resultant is simply: = Resultant = = 2 T1 + 2 T2 04 ( ) ( ) Continue to lesson 13b after completing this exercise. 13a-22 MSC.Nastran 105 Exercise Workbook