Problem: Model a cantilevered beam using plate elements subjected to a constant tip loading. The plate elements will undergo bending. With plate material: Aluminum with E = 10 x 10^6 psi and n =0.3. With a load on tip of plate = 8 lbf. Finally, display the von Mises stress and the deformed shape of the plate model.
Horizontal spacer

1) Click Structures

1) Select Tools and click on Options.

2) Highlight Units Manager…

3) Click on Standard Units.

4) Scroll down and select the line with units in, lb, s,…

5) Click OK. .

1) Under Workspaces, expand Structures then Entity Options.

2) Highlight FEA Symbols Structures.

3) For Labels, select None and check Show LBC Value

4) Click OK on the User Options form.

1) Under the Geometry tab, select Filler from the Surface group.

2) Click on points.

3) Click in the Entities text box. And enter 0,0,0;5,0,0;5,1,0;0,1,0.

4) Hit enter then Click OK on the Filler form.

5) Click Fill on the View Manipulation toolbar.

1) Under the Materials and Properties tab, select Isotropic from the Material group.

2) Enter Aluminum for Name.

3) Enter 10e6 for Young’s Modulus.

4) Enter 0.3 for Poisson’s Ratio.

5) Click OK.

1) Click on Shell in the 2D Properties group.

2) Enter Al Plate for Name.

3) Click in the Entities text box, Select the surface.

4) Click in the Material text box then select Aluminum from the Model Browser.

5) Click in the Part thickness text box and enter 0.1.

6) Click OK.

1) Under the Meshing tab, select Surface from the Automesh group.

2) For Surface to mesh select the surface in the window.

3) Click OK.

1) Under the LBCs tab, select Force from the Loads group.

2) For Name enter 8 lb.

3) Click in the Entities text box and select the node at the far right corner as shown.

4) For Magnitude enter 8.

5) The direction of the force is in the negative z-direction. Enter -1 in Direction-Z text box.

6) Click OK.

7) Turn On Detailed Rendering.

1) Select Fixed from the Constraints group.

2) Enter Fixed for Name.

3) Click in the Entities text box.

4) Select Pick Curves from the Pick Filters.

5) Click on the Pick Nodes icon on the Pick Filters to deselect.

6) Select the curve at the left end of the plate.

7) Click OK.

1) Right click on FileSet and select Create new Nastran job.

2) Click on the folder icon for Solver Input File. Navigate to a location to save the analysis files.

3) Click OK.

4) Right click NewJob and select Run.

1) Select File then choose Attach Results.

2) Click the folder icon.

3) Navigate to and select the file newjob.xdb.

4) Click Open.

5) Select Results for Attach Options.

6) Click OK.

1) Under the Results tab, select Deformation from the Results group.

2) Select the Result Case.

3) For Result Type select Displacements, Translational.

4) Click the Deformation tab.

5) Check Show undeformed.

6) Click Update.

1) Click Hide.

2) Click the Plot Data tab.

3) Pull down Plot type to Fringe.

4) Select Stress Tensor for Result Type.

5) Select von Mises for Derivation.

6) Click Update.