 Hello students, I welcome you all to this session on finite element method and in this session we are going to look at the static structural analysis of a cantilever using finite element commercial package. I am Deepak Maslaker working as assistant professor in the department of mechanical engineering at WIT Solapur. Learning outcomes of this session are at the end of this session students will be able to understand what is the meaning of static structural analysis, what is the significance of static structural analysis and how to solve a problem by using ANSYS which is a finite element software. What is the meaning of static structural analysis? The meaning of word static is body is at rest and in static structural analysis we try to investigate displacement, strain, stress when the body is at rest and subjected to external forces which are independent of time. So, when the body is acted upon by forces and the body is at rest, what is the displacement at various points on the body? What are the stresses at different sections? What are the values of strains that we try to investigate in static structural analysis and when should know why this analysis is necessary because with the help of static structural analysis we can find out the stresses and from theories of failure it is well known that when the stress at a point in the loaded body becomes more than some threshold value then failure may occur and in order to avoid failure we should keep the stresses and strains within the body within a certain limit and therefore it is quite necessary to estimate the stresses, strains and displacements so that the values of stress, strain and displacement should not cross certain threshold. Let us now look at a problem. Here is a problem related with a cantilever beam. We have a cantilever of length 250 mm, diameter 50 mm and Young's modulus of the beam material is 200 GPa. At the free end of the cantilever we have applied a transverse load 3 kN, axial load 15 kN and a moment 1000 Nm and we are interested in the resultant stress at A, resultant stress at B, principal stresses, maximum shear stress and bending stress. These parameters are to be investigated. So let us go to ANSI's workbench. Here is the graphical user interface of ANSI's workbench. Now here I am selecting static structural analysis. So you double click on a static structural. Now let us define material and I call this material as material 1. So I am giving the name to the material as material 1. Let us define isotropic elasticity. Young's modulus is how much is the Young's modulus that is 200 GPa. So this is 2109 Pa. Let us say Poisson's ratio is 0.3. Once material property is defined I go to project schematic, double click on geometry. Now I choose XY plane and I change the unit to millimeter. Length of the beam is 250 mm. Please keep in mind length of beam is 250 mm. So I go to sketching, line, let us go to dimensions, general, click on the line and this line has length 250 mm. Let us convert this line into line body, modeling, go to concept, line from sketches. Now sketch is drawn in XY plane, sketch 1 is selected in XY plane. Apply line 1, generate. So what I have done, this line is converted into a line body. Let us assign cross section to this body. Let us assign cross section, concept, cross section, circular and what is the radius of this cross section? Radius of the circle, what is the radius of the circle? 25 because diameter is 50 mm, radius 25. Now I choose line body and to this line body I assign a circular cross section. Now I got a body having circular cross section. We can see this by going in view option, view, cross section solid and you can see this is isometric view. So we have generated this body. Let us minimize this window and go to model. So when I click on this ball, I will get isometric view. When I click on z axis, I will get XY plane. Let us assign the material. Here is geometry, line body. Now the default material in ANC is structural steel but I have a new material named as material 1. So I have assigned material 1 to this line body. I go to mesh, right click, generate mesh. Let us improve the quality of mesh by sizing option, resolution is made 5, right click on mesh, update the mesh. So I have increased the mesh density. Let us apply boundary condition, right click on static structural, insert a fixed support and I am going to put a fixed support at node, left node, fixed support, apply. So at the left node, I have applied a fixed support. Let us apply various loads at the free end. So again right click on static structural, apply force and force is to be applied at this node, apply. Instead of vector, just take components. The component in x direction is 15. Here you can see the force is x component is 15,000 Newton and now again I select right click on static structural. Here is force at this location, apply. Instead of vector, I should take component. The y component is 3 kilo Newton but in the negative direction minus 3000 Newton y component. So at the free end, two forces are applied. Let us apply one moment, right click on static structural, insert a moment. I am going to insert a moment and the moment is to be applied at this location, apply. Instead of vector, I should take components and the x component is 1000 Newton meter is the x component. Once we apply this moment, what we can do is the following. Right click on static structural and solve beam section results. Yes. Now I am going to insert, I am going to insert stress and this stress is shear stress. Then in the solution, I go for right click, insert, stress, normal stress, insert, stress, maximum principal stress, insert, stress, bending stress, insert, stress, normal stress, right click on solution and evaluate all results. Here you can see what is the maximum shear stress. The maximum shear stress is 4.08 into 10 to the power 7. It is in Pascal's. I change the unit. What I do for changing the unit, I go to home, tools, units and the units are metric mm. So I will get a stress in mega Pascal's. So maximum shear stress is 40.828 mega Pascal's minimum minus 40.828 mega Pascal's. Normal stress is maximum bending stress is 68. This is the resultant stress. This is minus 53.597. Here is maximum principal stress 87 minimum principal stress 7.6. So in this way, we have carried out the stress analysis. Thank you very much.