Problem: This problem involves using utilizing load cases to determine the internal moments of a simple frame that consists of two beam columns (AB and CD) that are 12 ft. and a beam (BC) that is 14 ft both of which are assumed to be W12 sections. Both supports are fixed. The beam is loaded with a uniform distributed load in of 2 k/ft in the negative y-direction in the first load case and a lateral load of of 20 k applied at the midpoint of beam AB in the positive x-direction in the second load case. An isotopic material (steel) of Elastic Modulus, 30E6, and Poisson Ratio, 0.3, is applied to the beams. The frame is then meshed with a Bar2 finite element mesh and processed with linear static analysis.

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

2) Type the name of the new database as Frame 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 Points and select XYZ.

2)Input the following point coordinates and click Apply after each point: [0 0 0], [0 144 0], [168 144 0], and [168 0 0]. There are no units in Patran, and therefore it is important to stay consistent in units.

3) Under the Geometry tab, click on Curves and select Point.

4) With Auto Execute checked, click on Point 1 then Point 2, Point 2 then Point 3, and Point 3 then Point 4.

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 Beam under the 1D Properties section.

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

3)Click on Select Material and select steel. Click OK.

4) Input <1 0 0> as the Bar Orientation, this ensures that the beams are oriented in the x-direction.

5) Click on Create Sections: Beam Library and input i_section for the New Section Name. Then input the properties of the W section: 18 for H, 12 for W1, 12 for W2, 0.5 for t, 0.5 for t1, 0.5 for t2. Then click Apply and then click Cancel. Make sure the Section Name has i_section selected if not, select it by clicking on the "I Beam" icon. Then click OK.

6) Click on Select Application Region and then click on the Select Members box. Screen pick Curves 1 and 3. Click Add, OK then Apply and then click Cancel.

7) Input horizontal_beam as the Property Set Name and then click on Input Properties .

8) Click on [Section Name] and select i_section. Click OK.

9) Click on Select Material and select steel. Click OK.

10) Input <0 1 0> as the Bar Orientation, this ensures that the beams are oriented in the y-direction.

11) Click on Select Application Region and then click on the Select Members box. Screen pick Curve 2. Click Add, OK then Apply and then click Cancel.

12) You can check to see if your beams are oriented properly by going to Display: Load/BC/Elem. Prop... and then under beam display choose 3D:Full Span. You can change it back to 1D: Line afterwards if you desire.

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>, and Rotations as <0,0,0>. Click OK.

4) Click on Select Application Region, in the selection toolbar, select Point. In the Select Geometry Entities, screen select Point 1 and Point 4. Click Add. Now click OK then Apply.

1) Under the Meshing tab, click on Uniform Mesh Seeds.

2)Set the Number of Elements to 2. Click on the Curve List box and screen select Curves 1, 2 and 3. Click on Apply.

3) Under the Meshing, click on Curve as Mesh and Type Curve.

4) Set the Topology to Bar2. Click on the Input List box and screen select Curves 1, 2, and 3. Set the Global Edge Length to Automatic Calculation. Click on Apply.

5) Set Action to Equivalence and click Apply (This will eliminate duplicate nodes at the intersection of two curves).

1) Click on Force. Enter New Set Name as lateral_force and click on Input Data.

2) Converting from kips to pounds, enter <20000,0,0> as the Force and click OK.

3) Click on Select Application Region and under Select choose FEM and select Node 2. Click Add and then OK and Apply and the 20 kip force should now be applied at the midpoint of beam column AB.

4) Click on the Element Uniform box and select Distributed Load. Enter New Set Name as distributed_load. Make sure Target Element Type is set to 1D and click on Input Data.

5) Converting from kip/ft to lb/in, enter <0,-166.67,0> as the Distr Load and click OK.

6) Click on Select Application Region and under Select choose Geometry and select Curve 2. Click Add and then OK and Apply and the 2 kip/ft distributed load should now be applied on Beam BC.

2) Enter lateral_load for the Load Case Name, then make sure Type is set to Static . Then click on Input Data.

3) Under Select Individual Loads/BCs Select Displ_Fixed and Force_lateral_force. It should then appear under Assigned loads/BCs. Click OK and then Apply.

4) Enter distributed_load for the Load Case Name, then make sure Type is set to Static . Then click on Input Data.

5) Under Select Individual Loads/BCs Select Displ_Fixed and Distr_distributed_load. It should then appear under Assigned loads/BCs. Click OK and then Apply.

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

2)Return to the Analysis tab, select Subcases.... Click on lateral_load under Available Subcases and then click on Output Requests....

3) Then under Select Result Type click on Grid Point Force Balance to add it to the Output Requests. GPFORCE=ALll FEM should be listed now under Output Requests. Click OK and Apply.

4)Return to the Analysis tab, select Subcase Select.... Click on lateral_load to add them to Subcases Selected. The only subcase that should be listed is lateral_load, if any other subcases are listed under Subcases Selected, then click on it to remove it from the list. Click OK and OK. Now you are ready to run this case by clicking Apply on the Analysis tab.

5) Return to the Analysis tab, input distributed_load for the Job Name and click Solution Type. Choose LINEAR STATIC. Click OK and OK.

6)Return to the Analysis tab, select Subcases.... Click on distributed_load under Available Subcases and then click on Output Requests.... Then under Select Result Type click on Grid Point Force Balance to add it to the Output Requests.

7) Then under Select Result Type click on Grid Point Force Balance to add it to the Output Requests. GPFORCE=ALll FEM should be listed now under Output Requests. Click OK and Apply.

8) Return to the Analysis tab, select Subcase Select.... Click on distributed_load to add them to Subcases Selected. The only subcase that should be listed is distributed_load, if any other subcases are listed under Subcases Selected, then click on it to remove it from the list. Click OK and OK. Now you are ready to run the model by clicking Apply on the Analysis tab.

1) Now change the Action to Access Results Object to Attach XDB.

2) Select lateral_load and go to Translation Parameters and check Rotational Nodal Results. Click OK and Apply.

3) Select distributed_load and go to Translation Parameters and check Rotational Nodal Results. Click OK and Apply.

4) Click the Results tab, select either lateral_load or distributed load to view the results for that load case then under Object select Freebody, and under Select Results Type you can select Constraint Forces to view the reactions at the supports.

5) To view the Internal Forces and Moments, click on Display Attributes in the Results Tab and under show, choose Force/Moment. Uncheck Mx and My and return to the Select Results tab. Under Select Results Type choose Internal Forces to view results.

6) To view the internal moments at the joints (as opposed to the previous step which showed us the Summation of the Internal Moments at the joints), simply click on Select Entities, the second icon from the left, and under Select Element, choose the desired element you wish to view the internal moment for, and click Add and Apply. Repeat the same process to find out the other internal moments. The internal moment BA for the distributed load case is shown below as an example.

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.

Also, we wanted to learn how to access the freebody diagram to view the external/internal forces and moments during post-processing.

We can check our work by applying the Slope-Deflection Method which will give us the analytical solution.

Since finite element analysis simply gives us approximate results, there will always be a discrepancy between the analytical, or exact, solution and the and results of a finite element analysis. We can achieve a more accurate solution be adding more finite elements to the meshing.

We can note this discrepancy in the second load case where the MD Nastran results do not give internal moments of zero at points B and C (since at equilibrium the sum of internal moments should be zero). However, as the mesh is refined with more finite elements, the internal moments at those points will converge to zero such as in the case below where 500 nodes are used for Beam BC.