Problem: Using Patran/MSC Nastran, determine the maximum nominal stress in a plate with dimensions of 2 in. x 4 in. x 0.25 in. that contains a hole with a radius of 0.1875 in. for a total load of 300 lb/in. that is applied on the right edge of the plate. The plate is fixed on the left edge.
Horizontal spacer

1) Click on New from the File menu or from the Defaults Toolbar as shown.

2) Type the name of the new database as Plate_with_hole and click OK.

3) In the Approximate Maximum Model Dimensions box, input 10.0. Choose Structural for the analysis type. Click OK.

1) Under the Geometry tab, click on Solids and select Primitive.

2) Choose Block, then input the following Block Parameters (X length = 4, Y length = 2, Z length = 0.25) and input [-2 -1 0] for the Base Orgin then click Apply. There are no units in Patran, and therefore it is important to stay consistent in units. (If Auto Execute is checked all you have to do is hit enter, do not click Apply, and it will create the geometry for you. Be careful not to create duplicate solid geometries.)

3) Then choose Cylinder and input 0.25 for the Height list, 0.1875 for the Radius list, 0.0 for the Thickness List and [0 0 0] for the Base Center Point list. Then click Apply.

4) Then under Action, select Edit, under Object, select Solid, and under Method, select Boolean. Then click on Subtract (the middle icon) and under Target Solid, screen select Solid 1 (The whole Block), and under Subtracting Solid List, screen select Solid 2 (the Cylinder).

5) You can verify that the Boolean has been done correctly by right-clicking anywhere in the background and going to Viewport Display and then Smooth Shaded. Once you've done that, revert the Viewport Display back to Wireframe.

1) Under the Properties tab, select Isotropic.

2) Input steel as the Material Name and then select Input Properties.

3) Input Elastic Modulus = 30E6, Poisson Ratio = 0.3. Click OK and Apply.

1) Click on Solid under the 3D Properties section.

2) Input plate as the Property Set Name and then click on Input Properties ....

3) Click on Select Material and select steel. Under Thickness, input 0.25. Click OK.

4) Click on Select Application Region and then click on the Select Members box. Screen pick all members. Click Add, OK

1) Under the Load/BCs tab, select Displacement Constraint.

2) Input New Set Name as the Fixed, and click on Input Data.

3) Enter Translations as <0, 0, 0>. Click OK.

4) Click on Select Application Region click on the Surface or Face. For the Application Region, screen select the left surface/face of Solid 1 as shown. Click Add, now click OK then Apply.

1) Click on Total Load. Enter Load as New Set Name. Make sure the Target Element Type is set to 3D. Click on Input Data....

2)Enter <600, 0, 0> as the Load and click OK.

3) Click on Select Application Region

4) Now, click on the Select Geometry Entries box. For the Application Region, screen select the right surface/face of Solid 1 as shown. Click Add, now click OK then Apply.

1) Under the Meshing tab, select Uniform under Mesh Seeds.

2) Enter 12 as the Number of Elements and under Curve List, screen select the two curves that compose the hole. Then click Apply.

3) Now under the Meshing tab, set the Object as Mesh and Type as Solid.

4) Set the Elem Shape to Tet and Topology to Tet4. Click on the Input List box and screen select the entire solid.

5) Uncheck Automatic Calculation and set the Global Edge Length to 0.25. Click on Apply.

1) Under the Analysis tab, select Entire Model. Input Plate_with_hole for the Job Name. Click Solution Type. Choose LINEAR STATIC.

2)Click Solution Type. Choose LINEAR STATIC.

3) Now click on Subcases... and for the Available Subcases choose Default and click on Output Requests.

4)Under Output Requests make sure that STRESS(SORT1,REAL,VONMISES,BILIN)=All FEM;PARAM,NOCOMPS,1 is listed. Click OK, Apply.

5) Now you are ready to run the model by clicking Apply on the Analysis Tab.

1) Now click on XDB.

2) Ensure the appropriate Job Name is selected and click Apply.

3) Click the Results tab, select Fringe/Deformation for Object. Choose Displacements, Translational for Select Deformation Result, then click on Fringe Attributes.

4) Click on Select Results, for the Select Fringe Result, choose Stress Tensor. For the Select Deformation Result choose Displacements, Translational then click Apply.

In this example, we wanted to focus on learning how to assign beam properties (such as beam section dimensions, beam orientations, and material properties) and set up multiple load cases with Patran during pre-processing.

The average stress can simply be calculated first and multiplying it by the Stress Concentration Factor, Kc, will give us the maximum stress in the system.