 Hello friends, my name is Saurabh Deshmukh, working as an assistant professor in Department of Mechanical Engineering, Volchian Institute of Technology, Solapur. In this video, we are going to perform the static structural analysis of a cantilever beam using APDL, the learning outcome. After the end of this session, the learner will be able to perform analysis of cantilever beam using link 180 element. So we have opened the APDL window here. So first of all, we will need to choose the preferences. Just click on the preference, the new tab will open. So we are going to perform the structural analysis here. So click on that and just click on OK. So after that, click on the pre-processor. Then we need to select the element type. So click on the element type, then add, edit, delete option. You will find here. So click on that element, then click on the add. We are going to choose the link element here. So click on the link and 3D finest range 180 link you will find here. So just click on the OK. Now close this window. Now the real constants. But we are using here ansys 2021 version. So the real constants for the link 180 elements are not supported for the latest version of ansys. So you will find it here. Just click on the real constant, add here. Just click on the link 180 and just click on the OK. You will find the real constant for the link 180 element type are no longer supported here. So we need to create the link here. So first of all that, we will use the material properties. So click on the material property. Just click here on the material models. Then for the structural linear elastic, we are going to select the structural seal. So it will be isotropic. So the Young's modulus for the structural seal is 2E5, 2 into 10 raise to 5. That is Newton per mm square and the Poisson's ratio is 0.3. So click on the OK. You will find here the material is here, we have created a material. So just click on the close button. Now go to the modeling. Create key points. Now we are going to use the key points in the active coordinate system. Just click on the active coordinate system. There is no need to give the key point number. The answers by default take it in the sequence that is 1, 2, 3, 4. So there is no need to assign the values here. And you will find three sections here for x, y, z location in active coordinate system. So first is of x coordinate, second is of y coordinate and third is of z coordinate. So by default, if we click on the apply button, it will be taken as 0. So obviously the first element we are going to take at origin. So we will directly apply here. Then for the second element, it is at 300 mm. So just click, just right here, 300 mm, apply. And the third key point will be at 700 mm away from the origin. So it will be taken as a 700, apply. And the fourth key point is at 1000 mm away from the origin. So it will be 1000. Okay, just click on the apply and close it. You'll find the four key points are formed here. We have created four key points. Now we are going to create the lines. So click on the lines, a line and straight line. Click on the first key point to second. The first line is formed. The second to third and third to fourth. Just click on the OK button. Now we need to create the links here. So go to the sections. You will find option link because we can't give the real constant. That is area for the beams here. So click on the link, then add. We need to create three links here for three different step bars. We have studied in the previous problems, okay, previous video. So the first link, just give the, for the first step bar, give the one ID here. So click on the OK, then click on one and you will find here section data that is link area. Okay, so the first area of the link is 300 mm square. So click on the OK. Then we need to add another element. I just click on the add. Now we need to give the different ID name here. So we will click here, we will write here two, okay, then two again and the area of the second beam is 200 mm square. Just click on OK and then for third link, we need to give here three, okay, then three and the area of the third beam is 90 mm square. So we have written here 90 in the box of link area. So click on the OK here. We have created three links for three different bars. Now we need to mesh these lines here. Before that, we need to apply the area, okay, so go to the mesh attributes, then click on the lines, picked lines, then select the first line, click on the OK. You'll find here the material number, okay, the material is uniform for all the beams. So we'll keep it as one, then link 180, we are going to perform the analysis using link 180. There is no problem. Just we need to here select the element section, okay. The first section is of 300 mm square, mm square area. The second section is of 200 mm square area and third section is of 90 mm square area. So the first line is of 300 mm square. So just click and click on the up line, okay. Then select the second line, just click on the OK here. Then we need to select here second element, okay, element section of 200 mm square cross-sectional area. Just click and apply, then select the third line to apply the 90 mm square section here, okay, and then click on third, just click on the OK. So we have applied different areas for the different lines. Now we have applied the area. Now we need to mesh these lines, okay. Just click on the mesh tools, you'll find here a dialog box. Now we will divide these lines into one element, okay, because we are going to find the nodal values. So at first node, second node, third node and fourth node. So we need to mesh these lines or discretize these lines into one element. So just you'll find here line section. So select on the set, click all the three lines, click on OK. You'll find either we can give the length, edge, element, edge length or number of element division. So we will divide the lines into one element. So we will click here and apply here one, then click on OK. Then again go to the mesh tool. Just click here on the mesh button, select all three lines to machine it and OK. So we have meshed the lines here. Now we are going to apply the boundary conditions, okay. So the loads, define loads, apply, you'll find a structure here, structural, then displacement, okay. So we can choose here either key points or not because the key points are only nodes here for the elements, okay. So though we will select on the key points here, we are going to fix this support, okay. So click on the key point here, click on the OK. The new dialog box will get open and here we will find the degrees of freedom to be constrained. So we are going to constraint all degrees of freedom. So click on the all and click OK. So you will find here we have constrained this key point here or node here. So now we will apply here the force of 50 kilo Newton as we have discussed in earlier video. So click on the force oblique moment, on the key point, just select key point, then click on the OK. You'll find the direction of force or momentum, okay. So in f of x, f of y and f of z, we are going to apply in the direction of x axis. So we'll keep it as f of x and then 50 kilo Newton that is 50 into 10 raise to 3, okay. So click on the OK. So we have applied here a force of 50 kilo Newton. So we are going to now solve this problem, go to the solution, solve, you'll find two option current load step and from load step files. So we can give the different load step in a PDL but for this problem we have we have chosen only one load step. So just click on the current load step, click on OK. The solution is done here, close the dialog box. Now we will see the results here, the deformation, okay. So go to the list results, we are going to we are going to calculate the nodal values, okay. So click on the nodal solutions, then degrees of freedom solution. Obviously we have applied the force in x direction. So we are going to find the calculate or find the x component of displacement, okay. So we have selected it and click on OK. So you'll find it here the first displacement is 0 because we have constrained it for the second node it is 0.25 mm for the second for the third node it is 0.75 mm and for the third node it is 1.5033 mm. So these are we have calculated these values analytically in previous video you can check the link in the description and you will also find the maximum deformation value. So it is occurring at node 4 and its value is 1.5 mm, okay. I hope you have understood how to perform the structural analysis using APDL. These are the references, thank you.