WS12a-1 WORKSHOP 12A NORMAL MODES ANALYSIS FOR PRESTIFFENED PLATE MODEL USING SOL 103 OR 106 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software. - презентация

1 WS12a-1 WORKSHOP 12A NORMAL MODES ANALYSIS FOR PRESTIFFENED PLATE MODEL USING SOL 103 OR 106 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation

2 WS12a-2 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation

3 WS12a-3 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation n Problem Description u The purpose of this workshop is to demonstrate the ability of performing a normal modes analysis for a prestiffened structure using MSC.Patran and MSC.Nastran. In this workshop, a 1x1 square aluminum plate under tension loading is used. The goal is to do the following cases. l Perform a standard normal modes analysis using SOL 103 l Perform a normal modes analysis for prestiffening using SOL 103 l Perform a normal modes analysis for prestiffening using SOL 106 l Compare the natural frequencies and mode shapes for these three analyses.

4 WS12a-4 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation n Suggested Exercise Steps 1. Create a 1x1 surface. 2. Mesh the surface. 3. Create the boundary conditions. 4. Create the load. 5. Create the material. 6. Assign physical properties to the plate elements. 7. Perform a normal modes analysis (SOL 103) without pre-load. 8. Perform a normal modes analysis using the stiffness matrix from a linear static analysis (SOL 103). 9. Perform a normal modes analysis using the stiffness matrix from a nonlinear static analysis (SOL 106). 10. Attach the.XDB results files generated by the analyses. 11. Display the results using Quick Plot.

5 WS12a-5 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation CREATE NEW DATABASE Create a new database called ws12.db. a.File / New. b.Enter ws12 as the file name. c.Click OK. d.Choose Default Tolerance. e.Select MSC.Nastran as the Analysis Code. f.Select Structural as the Analysis Type. g.Click OK. a b c d e f g

6 WS12a-6 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 1. Geometry: Create / Surface / XYZ Create a geometry surface with dimension of 1 x 1. a.Geometry: Create / Surface / XYZ. b.Enter for the Vector Coordinate List. c.Click Apply. a b c

7 WS12a-7 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 2. Finite Element: Create / Mesh / Surface Create a finite element model of the surface. a.Elements: Create / Mesh / Surface. b.Select Quad Element Shape and IsoMesh Mesher. c.Select Surface 1. d.Uncheck the Automatic Calculation. e.Enter 0.1 for the Global Edge Length. f.Click Apply. a b c f d e

8 WS12a-8 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 3. Loads/BCs: Create / Displacement / Nodal Create the boundary condition. a.Loads/BCs: Create / Displacement / Nodal. b.Enter constraint_bottom for the New Set Name. c.Click on the Input Data button. d.Enter for Translations and for Rotation. e.Click OK. f.Click on Select Application Region. g.Change the Geometry Filter to FEM. h.Select the nodes along the bottom edge of the plate. i.Click Add, and click OK. j.Click Apply. a b c d e f g h i j i

9 WS12a-9 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 3. Loads/BCs: Create / Displacement / Nodal (Cont.) Create the boundary condition (cont.). a.Loads/BCs: Create / Displacement / Nodal. b.Enter constraint_left for the New Set Name. c.Click on the Input Data button. d.Enter for Translations and for Rotation. e.Click OK. f.Click on Select Application Region. g.Change the Geometry Filter to FEM. h.Select the nodes along the left edge of the plate. i.Click Add, and click OK. j.Click Apply. a b c d e f g h i j i

10 WS12a-10 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 3. Loads/BCs: Create / Displacement / Nodal (Cont.)

11 WS12a-11 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 4. Loads/BCs: Create / Total Load / Element Uniform Create the loads. a.Loads/BCs: Create / Total Load / Element Uniform. b.Enter right for the New Set Name. c.Change Target Element Type to 2D. d.Click on the Input Data button. e.Enter for the Edge Load. f.Click OK. g.Click on Select Application Region. h.Change the Geometry Filter to FEM. i.Select the elements along the right edge of the plate. j.Click Add, and click OK. k.Click Apply. a b c d e f g h i k j j

12 WS12a-12 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 4. Loads/BCs: Create / Total Load / Element Uniform (Cont.) Create the loads (cont.). a.Enter top for the New Set Name. b.Click on the Input Data button. c.Enter for the Edge Load. d.Click OK. e.Click on Select Application Region. f.Change the Geometry Filter to FEM. g.Select the elements along the top edge of the plate. h.Click Add, and click OK. i.Click Apply. a b c d e f g h i h

13 WS12a-13 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 4. Loads/BCs: Create / Total Load / Element Uniform (Cont.)

14 WS12a-14 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 5. Materials: Create / Isotropic / Manual Input Create the material. a.Materials: Create / Isotropic / Manual Input. b.Enter Al for the Material Name. c.Click on the Input Properties button. d.Enter 10e6 for Elastic Modulus and 0.33 for Poisson Ratio. e.Enter for the Density. f.Click OK. g.Click Apply. a b d c e f g

15 WS12a-15 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 6. Properties: Create / 2D / Shell Assign physical properties to the plate. a.Properties: Create / 2D / Shell. b.Enter plate for the Property Set Name. c.Click on the Input Properties button. d.Click on Material Prop Name icon, and select Al in the Material Property Set box on the bottom. e.Enter for the Thickness. f.Click OK. g.Select Surface 1 for the application region. h.Click Add. i.Click Apply. a b d c e f g h i d

16 WS12a-16 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 7. Normal Modes Analysis W/O Pre-load Using SOL 103 Submit the model for normal modes analysis. a.Analysis: Analyze / Entire Model / Full Run. b.Enter normal_mode for the Job Name. c.Click on Solution Type. d.Select NORMAL MODES. e.Click on Solution Parameter button. f.Enter for Wt-Mass Conversion. g.Click OK. h.Click OK. i.Click Apply. a b c d e g h f i Analysis 1: Normal modes analysis using SOL 103

17 WS12a-17 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Submit the model for normal modes analysis. a.Analysis: Analyze / Entire Model / Analysis Deck. b.Enter normal_mode_prestiff for the Job Name. c.Click on Solution Type. d.Select LINEAR STATIC. e.Click on Solution Parameter button. f.Enter for Wt-Mass Conversion. g.Click OK. h.Click OK. i.Click Apply. a b c d e g h f i Analysis 2: Normal modes analysis for prestiffened plate using SOL 103 Step 8. Normal Modes Analysis W/ Pre-load Using SOL 103

18 WS12a-18 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Examine the.bdf file generated from this analysis. a.Change the Solution Type from SOL 101 to SOL 103. b.Add the second subcase to include the STATSUB and METHOD statement. c.Insert the EIGRL command line into the Bulk Data section. b c a Step 8. Normal Modes Analysis W/ Pre-load Using SOL 103 (Cont.)

19 WS12a-19 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Execute the Nastran analysis outside of MSC.Patran. a.Select the normal_mode_prestiff.bdf from the window. b.Click on Open. c.Type scr=yes in the Optional Keywords section. d.Click Run. b c d a Step 8. Normal Modes Analysis W/ Pre-load Using SOL 103 (Cont.)

20 WS12a-20 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Submit the model for normal modes analysis with prestiffened condition. a.Analysis: Analyze / Entire Model / Full Run. b.Enter prestiffen for the Job Name. c.Click on Solution Type. d.Select NONLINEAR STATIC. e.Click on Solution Parameters button. f.Enter for Wt-Mass Conversion. g.Click OK. h.Click OK. a b c d e g h f Analysis 3: Normal modes analysis using SOL 106 Step 9. Normal Modes Analysis Using Nonlinear SOL 106

21 WS12a-21 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Submit the model for normal modes analysis with prestiffened condition (cont.). a.Click on Subcases… b.Enter prestiffen for the Subcase Name. c.Click on Subcase Parameters. d.Enable the Normal Modes option. e.Click OK. f.Click Apply. g.Click Cancel. b c d e a f g Step 9. Normal Modes Analysis Using Nonlinear SOL 106 (Cont.)

22 WS12a-22 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Submit the model for normal modes analysis with prestiffened condition (cont.). a.Click on Subcase Select… b.Select prestiffen and unselect Default. c.Click OK. d.Click Apply. b c d a Step 9. Normal Modes Analysis Using Nonlinear SOL 106 (Cont.)

23 WS12a-23 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 10. Analysis: Access Results / Attach XDB / Result Entities Attach the XDB result files. a.Analysis: Access Results / Attach XDB / Result Entities. b.Select normal_mode in the Available Jobs field. c.Click on Select Result File. d.Select normal_mode.xdb. e.Click OK. f.Click Apply. a b c d e f

24 WS12a-24 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 10. Analysis: Access Results / Attach XDB / Result Entities (Cont.) Attach the XDB result files (cont.). a.Select normal_mode_prestiff for Job Name. b.Click on Select Results File. c.Select normal_mode_prestiff.xdb. d.Click OK. e.Click Apply. a b c d e

25 WS12a-25 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 10. Analysis: Access Results / Attach XDB / Result Entities (Cont.) Attach the XDB result files (cont.). a.Select prestiffen for Job Name. b.Click on Select Results File. c.Select prestiffen.xdb. d.Click OK. e.Click Apply. a b c d e

26 WS12a-26 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 11. Results: Create / Quick Plot Create a Deformation and Fringe plot of the first mode of the Normal Modes analysis. a.Change the view to Iso View 3. b.Results: Create / Quick Plot. c.Select the A1:Mode 1. d.Select Eigenvector, Translational in both Result boxes. e.Click Apply. b c d d a e Without editing the.bdf file Solution 103 does not take the applied loads into consideration

27 WS12a-27 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 11. Results: Create / Quick Plot (Cont.) Create a Deformation and Fringe plot of the first mode of the prestiffened Normal Modes analysis. a.Select the A2: Mode 1. b.Select Eigenvector, Translational in both Result boxes. c.Click Apply. b b a c

28 WS12a-28 NAS122, Workshop 12a, August 2005 Copyright 2005 MSC.Software Corporation Step 11. Results: Create / Quick Plot (Cont.) Create a Deformation and Fringe plot of the first mode of the prestiffened Normal Modes analysis. a.Select the A3: Mode 1. b.Select Eigenvector, Translational in both Result boxes. c.Click Apply. b b a c