 Hello students. I welcome you to all to this session on finite element method. I am Deepak Maslaker, working as assistant professor in the department of mechanical engineering at WIT, Solapur. In this class, we are going to discuss about model analysis using finite element commercial package. Learning outcomes of this session are, at the end of this session, students will be able to understand what is the meaning of model analysis, what is the significance of model analysis and how to solve the problem related with model analysis using ANSYS. Let us understand what is model analysis. In model analysis, we try to find out the natural frequencies and more shapes of a vibratory system. When a system is vibrating at its own, that is, when a system vibrates due to its elastic properties, then the corresponding frequencies with which the system is vibrating are called as natural frequencies. And the corresponding modes are called natural modes or normal modes. And in model analysis, we try to investigate with what frequency the body is vibrating. And it is extremely important in the design to know what are the natural frequencies of a system. Because when the frequency of external excitation matches with the natural frequency of vibration, then that particular condition is called resonance. And when the body is in resonance, then it vibrates with maximum amplitude. And at resonance, there is a chance of a catastrophic failure of the system. And therefore, while designing a machine element, it is quite necessary to avoid the external excitation whose frequency should not be equal to the whose frequency is equal to the natural frequency of the system. Let us now try to understand how to solve a problem by using ANSYS. Here is the problem statement. And we are asked to determine first three natural frequencies and more shapes of a simply supported beam of 3 centimeter diameter, 1.5 meter long, density 7780 kilogram per meter cube, and Young's modulus 208 giga Newton per meter square. And Poisson's ratio for the beam material is given as 0.3. In order to solve the above problem, let us now go to ANSYS workbench. And in the graphical user interface of ANSYS workbench, you select the option of modal. And after choosing this modal option, a window will pop up in the project schematic. Here is engineering data. And I am going to define the material, material 1. Let us define properties of this material like density. Density of the material is 7780 kilogram per meter cube, material 1, isotropic elasticity, double click, that is 208 into 10 to the power 9 Pascal's Poisson's ratio 0.3. Material properties are defined. Now go to project schematic, open geometry. Now, I choose XY plane. Here is XY plane selected. And let us take the unit as centimeter. The maximum range that I am going to take is 200. Go to sketching, straight line and go to dimensions, general dimensions, length 150 centimeter. That is nothing but 1.5 meters. Let us convert this line into line body, modeling, go to concept, line from sketches. Sketch is drawn in XY plane. This is sketch 1, line selected, apply. Now the line is converted into line body, select the line and generate this line. Line has been converted into line body. Let us apply cross section to this line body concept, cross section circular. The circle has radius 1.5 centimeter because the diameter is 3 centimeter. Then go to line body, cross section is not defined, cross section is circular. You can see this body in the view option, cross section solid. Now this body, you can see this body as a solid body by using isometric view as a solid body. Once we complete this solid modeling, we go towards the option of model. Now I select geometry, line body and for the line body, the default material is structural steel. Instead of that, I am going to take material 1 as the material. So line body is now made up of material and the name of material is material 1. Here you can see material 1. After that, go to mesh, right click, generate mesh. Let us improve the quality of mesh, sizing, resolution. Resolution is made 5. Then go to mesh, right click, update mesh. Now the mesh has been updated. Let us apply boundary conditions. For that click on model, right click, insert remote displacement. I choose a node, boundary node is chosen, apply no displacement in x direction. So x component 0, no displacement in y direction. No displacement in z direction. Rotation about x is 0. Rotation about y is 0. But the body is allowed to rotate about z axis. Similarly, model, right click, insert remote displacement. Select the node, apply x displacement is 0. Displacement in y direction is 0. Displacement in z direction is 0. Rotation about x axis is 0. Rotation about y axis is 0. And the body is free to rotate about z axis. After applying boundary condition, right click and solve. It will take some time to solve. Here is the option, right click and then solve. So we have obtained the solution. Just click on the solution. And now you can see that the frequencies are 27 hertz, 61 hertz, 108 hertz, 168 hertz. These are the frequencies. I select all the frequencies here, right click, create more shapes. Then right click on the displacement, right click on the solution, evaluate all results. Now you can see that these are the natural frequencies like 27, 61, 108, 168, 242. These are the natural frequencies. Now we can see more shapes, total deformation. This is the first mode. The body is vibrating like this. This is the first mode of vibration. Here is the third mode of vibration. You can simulate this. But if you look at the second mode of vibration in the second mode, this beam is vibrating axially. But we are not looking at the axial vibrations of the beam. Just we are focusing on the transverse vibration of the beam. So I am considering mode number three, which is the transverse mode of vibration. And here is mode number five in the fifth mode. This is the vibrating condition of the body. And natural frequency of the fifth mode is 242.42 hertz. So in this way, we have determined the natural frequencies and mode shapes of transverse vibrations of a simply supported beam. So thank you very much.