1) Click on Solid under the 3D Properties section.
2) Input hook as the Property Set Name and then click on Input Properties ...
3)Click on Select Material and select steel. Click OK.
4) Click on Select Application Region and then click on the Select Members box. Screen pick all solids. Click Add, OK then Apply.
1)Under the Load/BCs tab, select Displacement Constraint.
2) Input New Set Name as the Hold, 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 click on the Surface or Face. For the Application Region, screen select the top of the hook as shown. Click Add. Now click OK then Apply.
1) Under the Meshing tab, click on Solids and set the Object as Mesh and Type as Solid.
2) Set the Elem Shape to Tet and Topology to Tet10.
3) Click on the Input List box and screen select the all Solids. Uncheck Automatic Calculation and set the Global Edge Length to 0.5. Click on Apply (This step may take a few minutes).
4) Set Action to Equivalence and click Apply (This will eliminate duplicate nodes at the intersection of two curves).
1) Click on Force.
2)Enter New Set Name as Force and click on Input Data...
3) Enter <0,-5000,0> as the Force and click OK.
4) Click on Select Application Region
5) Now,Click on the Select Geometry Entries box. In the filters toolbar, select FEM. Screen select the node that corresponds to the center of the radius/center of the thickness of the hook to apply the force there as shown. Click Add, OK then Apply.
1) Under the Analysis tab, select Entire Model. Input hook 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)Now go back to the Home tab and under Misc. click on Plot/Erase. Under Selected Entities, select the nodes that comprise of the rectangular portion of the hook as shown. Then click Erase and OK.
4) Click the Results tab, under Result Plots select Graph.
5) Under Select Y Result, select Stress Tensor, under Quantity select Y Component, and under X select Path Length.
6) Then Click on Select Entities (2nd icon from the left). Under Select Path Points, Hold Shift while selecting the first point, which is the midpoint of the section that lies on the inner radius of the hook and the second point which is the midpoint of the section that lies on the outer radius of the hook as shown. Then click Apply and Apply and the Stress Distribution Graph for you have created for the cross section should appear.
7) You can verify the numbers on the graph by clicking Cursor, under Result Plots, and then under Select Cursor Result click on Stress Tenor and under Quantity select Y Component and click Apply. Now you can click on any node to view the stress values at those points.