Workshop 9-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 9 Buckling Analysis of Plate. - презентация

1 Workshop 9-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 9 Buckling Analysis of Plate

2 Workshop 9-2 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 9 (cont.) 1. Model description a.The model dimension is 20 inch by 8 inch b.The following boundary conditions are applied to the model: Pin at the left end Rollers at the right end Zero vertical deflections at top and bottom edges c.Apply 100psi compressive loads at the right edge Total loads at right edge = (100) (8) (.01) = 8 Apply 1 lb each at grid points 11 and 55 Apply 2 lbs each at grid points 22, 33, and 44

3 Workshop 9-3 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 9 -- Boundary Conditions Simply supported Supported on rollers Supported in the Vertical Direction

4 Workshop 9-4 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 9 -- Applied Loads

5 Workshop 9-5 NAS101 Workshops Copyright 2001 MSC.Software Corporation Create the first surface a.Create / Surface / XYZ. b.Enter for the Vector Coordinate List. c.Use [0 0 0] as the Origin Coordinate List. d.Click Apply. Step 1. Create Geometry: Create/Surface/XYZ

6 Workshop 9-6 NAS101 Workshops Copyright 2001 MSC.Software Corporation Create mesh seeds that will be used to guide the mesh. a.Create / Mesh Seed / Uniform. b.Input 4 in the Number of Elements. c.Select Surface 1.1 as the Curve List. d.Click Apply. e.Input 10 in the Number of Elements. f.Select Surface 1.4 as the Curve List. g.Click Apply. Step 2. Finite Element: Create /Mesh Seed/Uniform Surface 1.1 Surface 1.4

7 Workshop 9-7 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2A. Finite Element: Create /Mesh/Surface Create surface mesh based on the mesh seeds assigned in the previous steps. a.Create / Mesh / Surface. b.Select Quad as the Elem Shape. c.Select IsoMesh as the Mesher. d.Enter Surface 1 for Surface List. e.Click Apply.

8 Workshop 9-8 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3. Material: Create /Isotropic/ Manual Input Create the material aluminum. a.Create / Isotropic / Manual Input. b.Type in alum for the Material Name. c.Click on the Input Properties button to bring up the Input Option window. d.Enter 2.9E7 for the Elastic Modulus, and 0.3 for Poisson Ratio e.Click OK to return to the main material menu. f.Click Apply.

9 Workshop 9-9 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4. Element Properties: Create /2D/ Shell Create the element properties. a.Create / 2D / Shell. b.Enter plate as the Property Set Name. c.Click on the Input Properties button. d.Click on the alum in the Material field on the bottom section of the Input Properties window. e.Enter 0.01 as the thickness for the plate. f.Click OK. g.Select Surface 1 for the Application Region h.Click Add. i.Click Apply.

10 Workshop 9-10 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter simply_supported_left as the New Set Name. c.Click on the Input Data. d.Enter for the Translation field. e.Click OK. f.Click on Select Application Region. g.Select FEM as the geometry filter.. h.Select Node 1,12,23,34,45 for the Application Region.These are nodes along the left edge of the rectangle. i.Click Add. j.Click OK. k.Click Apply.

11 Workshop 9-11 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5A.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

12 Workshop 9-12 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter support_vertical_botto m as the New Set Name. c.Click on the Input Data. d.Enter for the Translation field. e.Click OK. f.Click on Select Application Region. g.Select FEM as the geometry filter.. h.Select Node 1 through 11 for the Application Region.These are nodes on the bottom i.Click Add. j.Click OK. k.Click Apply.

13 Workshop 9-13 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6A.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

14 Workshop 9-14 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 7. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter support_vertical_top as the New Set Name. c.Click on the Input Data. d.Enter for the Translation field. e.Click OK. f.Click on Select Application Region. g.Select FEM as the geometry filter.. h.Select Node 45 through 55 for the Application Region.These are nodes on the top edge of the rectangle. i.Click Add. j.Click OK. k.Click Apply.

15 Workshop 9-15 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 7A.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

16 Workshop 9-16 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 8. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.Create / Displacement / Nodal. b.Enter supported_rollers_rig ht as the New Set Name. c.Click on the Input Data. d.Enter for the Translation field. e.Click OK. f.Click on Select Application Region. g.Select FEM as the geometry filter.. h.Select Node 11,22,33,44,55 for the Application Region.These are nodes on the right edge of the rectangle. i.Click Add. j.Click OK. k.Click Apply.

17 Workshop 9-17 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 8A.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

18 Workshop 9-18 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 9. Loads/BCs: Create/Force /Nodal Apply distributed load to the model. a.Create / Force / Nodal b.Enter edge as the New Set Name. c.Click on the Input Data button. d.Enter in the Force field. e.Click OK. f.Click on Select Application Region button. g.Select FEM as the Geometry Filter. h.Select Node 11,55 for the Application Region. i.Click Add, and OK. j.Click Apply.

19 Workshop 9-19 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 9A.(cont.) Loads/BCs: Loading on the right edge After you have completed previous steps,then you see the load on the model as shown below:

20 Workshop 9-20 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 10. Loads/BCs: Create/Force /Nodal Apply distributed load to the model. a.Create / Force / Nodal b.Enter middle as the New Set Name. c.Click on the Input Data button. d.Enter in the Force field. e.Click OK. f.Click on Select Application Region button. g.Select FEM as the Geometry Filter. h.Select Node 22,33,44 for the Application Region. i.Click Add, and OK. j.Click Apply.

21 Workshop 9-21 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 10A.(cont.) Loads/BCs: All the loadings plus constraints After you have completed previous steps,then you see the loads and constraints on the model as shown below:

22 Workshop 9-22 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 11. Analysis: Analyze/ Entire Model/Full Run Submit the model for analysis. a.Analyze / Entire Model / Full Run. b.Click on the Solution Type. c.Select BUCKLING as the Solution Type. d.Click OK. e.Click on the Solution Parameters f.The menu called Solution Parameters is shown on next page

23 Workshop 9-23 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 12. Analysis: Analyze/ Entire Model/Full Run a.Uncheck the box label Large Displacements b.Click on Eigenvalue Extraction button. c.Extraction Method is Lanczos Put in number 5 for Number of Desired Roots. d.Click OK. e.Click OK f.Click OK g.Click APPLY

24 Workshop 9-24 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 13. Analysis: Attach XDB/ Result Entities/ Local Attach the XDB result file. a.Attach XDB / Result Entities / Local. b.Click on Select Result File. c.Select the file called w9. xdb d.Click OK. e.Click Apply.

25 Workshop 9-25 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 14. Results: Create/Quick Plot Create a Quick Plot of the results. a.Create / Quick Plot. b.Select SC2 result case. c.Select Eigenvectors, Translational for both the Fringe results and for the Deformation d.Click APPLY.