1) Click on Structures.

1) Select Tools > 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.

6) Click OK on the User Options form.

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

2) Check Points.

3) Click in the Entities text box. Enter 0,0,0;10,0,0;10,10,0;0,10,0,hit enter

4) Then click OK

5) Click Fill on the View Manipulation toolbar.

6) Pull down Geometry Wireframe on the Render toolbar.

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

2) Enter Aluminum for material Name.

3) Enter 10e6 for Young’s Modulus.

4) Enter 0.3 for Poisson’s Ratio.

5) Click OK.

1) Select Shell from the 2D Properties group.

2) Select part P1 in the Model Browser.

3) Click in the Material text box.

4) Select Aluminum from Model Browser.

5) Enter 0.1 for the Part Thickness.

6) Click OK.

1) Change the view to Top.

2) Under the Geometry tab, select Fillet from the Curve group. And select surface.

3) Click in the Vertices text box then select Select All from the Pick Filters.

4) Enter 1 for Blend Radius.

5) Click OK.

1) Select Washer 2 from the Features group.

2) Click on the model in the window.

3) Click in the Washer Hole Center text box and select Specify XYZ coordinates from the Pick Filters. Enter 2 2 0, then click OK.

4) Enter the following parameters: Hole Diameter: 1. Washer Diameter: 1.2. Num. Rings Beyond Washer: 3. Elem. Size Beyond Washer: 0.2. No. of Elements Around Hole: 16. No. of Levels: 2.

5) Click OK.

1) Select Washer 2 from the Features group.

2) Click on the model in the window.

3) Click in the Washer Hole Center text box and select Specify XYZ coordinates from the Pick Filters. Enter 2 2 0, then click OK.

4) Enter the following parameters: Hole Diameter: 1. Washer Diameter: 1.2. Num. Rings Beyond Washer: 3. Elem. Size Beyond Washer: 0.2. No. of Elements Around Hole: 16. No. of Levels: 2.

5) Click OK.

1) Under the Assemble tab, select RBE3 from the Interpolation Connectors group and choose basic.

2) Screen pick the nodes on the screen.

3) Check all 6 Reference Grid DOF.

4) Click OK.

1) Under the LBC’s tab, select Force from the Loads group.

2) Click in the Entities text box and select the node at the center of the hole.

3) Enter a force Magnitude of 5.0.

4) The direction of the force is to be in the global z-direction. Enter 1 for Direction Z.

5) Click OK.

1) Pull down Isometric View on the Model Views toolbar.

2) Click Fill on the View Manipulation toolbar.

3) To turn on the display of the force vector and labels: on the Render toolbar click on the Detailed Rendering On icon.

4) To modify the display of the Force vector, double click on Force_1 in the Model Browser.

5) Click the Visualization tab.

6) Change the % Screen to 20.

7) Pull down the color panel and select Blue.

8) Click OK

1) Select Pin from the Constraints group.

2) Enter Pinned for Name.

3) Click in the Entities text box and click Pick Nodes on the Pick Filter.

4) Click on Pick Surfaces to deselect it.

5) Pick one node on the outside edge of the plate.

6) Click OK.

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

2) Enter Plate_with_Hole for Job Name.

3) Click the folder icon to the right of the Solver Input File text box.

4) Click OK.

5) Right click on the simulation name Plate_With_Hole, select Run.

1) Select File > Attach Results.

2) Click the folder icon to the right of the File Path text box.

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

4) Click Open.

5) Click OK.

1) Under the Results tab select Fringe.

2) Select the Result Case.

3) For Result Type select Stress Tensor.

4) For Derivation select von Mises.

5) Click Update.

6) Hide the display of Boundary Condition Symbols.