2.31 Assignment 7 Due Mon, Oct 22 at 9:30 am A torsion pendulum consists of a solid rigid cylindrical disk of radius R=3m and height H=1m suspended by a shaft of length L=10m with a circular cross section of radius r=1m. The disk is subjected to an axial traction on its lower surface p=10 MPa, and a torque T=240MNxm. The material elastic properties are E=200 GPa, and ν=0.3. In order to avoid fatigue failure, the maximum principal stress (σ1) in the component must be limited to 300 MPa. Our task is to verify if the component meets the design requirements. 1) Pen and paper work (no FE) Calculate the maximum principal stress in the shaft subjected to the axial load resulting from p, and to the applied torque, T. A quick review of the formulas to calculate the principal stresses resulting from the superposition of shear and tension is attached at the end of this assignment. According to your calculations does the component meet the design requirement? 2) FE model Create a FE model of the component using linear full integration brick (3D stress) elements. Things to keep in mind as you set up the model: PART: You want to create a 3D Deformable Solid Part using Extrusion. Set the part approximate size to 10. Create the circular cross section of the shaft in the sketch tool (radius 1) and then extrude it by a length of 10. After you create the shaft, you add the disk by using the Create Solid: Extrude tool (also under ShapeÆ SolidÆ Extrude), extruding from the face at the bottom of the shaft, sketching a circle of radius 3 in the sketch tool, and then extruding (Blind) by a depth of 1. p T L rR HPROPERTY : In section property you want to create a solid homogeneous section of thickness 1. In material properties you have to input only the Mechanical props (E, ν). STEP : Choose static, linear perturbation. Do the mesh before you do the load! MESH : When you enter the mesh module the part looks orange because it cannot be automatically meshed. You must partition the part to help the mesh generator. 1) Separate the disk from the shaft using the ToolÆPartitionÆCellÆExtend Face tool, and clicking on the top face of the disk to extend it and partition the disk from the shaft. (Remember to click on create partition when the button appears!). 2)You also want to enforce symmetric meshes by creating partitions by splitting the parts in four quarters across reference (XZ, YZ) planes. The easiest way to do this is by creating two datum planes coinciding with the XZ, YZ reference planes, and then using them to split the part. The procedure is then: a) create the two datum planes ToolsÆdatumÆplaneÆOffset from principal planeÆApplyÆ choose YZ and Offset by 0.0 (if you centered the shaft at 0.0). Repeat to create an offset (by 0.0) of the XZ plane. Now you have two datum planes showing, and you can proceed with b) partitioning the cells : ToolÆPartitionÆCellÆ Use datum planeÆapplyÆselect the whole part (click and drag rectangle) Æselect a datum plane(XZ) by clicking on the edgeÆcreate partition. Repeat the thing with the other plane (YZ). Now your part is split and you can mesh it: SEED with size 0.5, Choose linear, full integration elements, mesh the whole thing. LOAD : Now you are ready to load the part. Create a pressure load (-10MPa) on the bottom plane of the disk (you will have to rotate the part to click on the correct plane. Remember to select all 4 quadrants of the bottom plane). Apply the torque as 8 concentrated forces acting counterclockwise, applied at the 4 +4 corners of the disk. (The corner points exist because you split the part with the daum planes). Encastre the top plane of the shaft. (All four quadrants!)Submit the job and look at the results in the VISUALIZATION module of ABAQUS/CAE: Plot the contours of Mises stress. Notice that they do not look quite right at the corner between the shaft and the disk: you expect a stress concentration right at the corner, but it is not there! This is because of the nodal averaging at of stresses, as the corner nodes also belong to the bulky disk elements. To see the real stress profile, you have to modify the defaults for field contours: In the ResultÆField Output window click on the Result option tag, and modify the nodal averaging threshold by moving the slider to 50%. ÆApply. Now you can actually see the stress concentration. Plot and print the Mises contours. Now plot and print the maximum principal stress(σ1). Note: this is not S11: it is one of the invariant stresses! Check the value of σ1 along the shaft away from the disk. Is it in agreement with your pen and paper calculation? What is the maximum σ1 in the component? Why is it so high? Does the component meet the design requirement? What could you do to improve the design and meet the