This tutorial describes the steps needed to create and analyze a model of a disk subjected to a temperature gradient and rotation. The first section describes the model building and application of a temperature gradient to compute nodal temperatures in the entire model. The second section describes the structural analysis with the computed nodal temperatures from the first section and a rotational velocity applied to the uncracked model. The third section describes the crack insertion and crack growth analyses using FRANC3D V5.0 and ANSYS.
Appendix A contains a comparison of results for an uncracked model using ANSYS and ABAQUS.
Building the Model in ANSYS for Heat Transfer Analysis
We will build the model using ANSYS. Start the ANSYS graphical user interface and select Preprocessor.
The first step is to define the element type. Select Element Type and then select Add/Edit/Delete. At this time, we can add both Solid87 and Solid92 element types; the first is for the heat transfer analysis and the second is for the subsequent structural analysis.
The next step is to define the material properties. Select Material Props Models and then select Material Models. We can define both the thermal and structural properties at this time. Material model #1 will consist of density, specific heat, enthalpy, thermal expansion and conductivity, and elastic modulus and Poisson ratio. The values can be temperature dependent, but for this analysis we will assume constant values for all temperatures.
The third step is to define the model geometry. Select Modeling and then select Create. First, we define keypoints in the active coordinate system (global Cartesian). We create keypoints at (0,0,0), (1,0,0), (10,0,0), (0,1,0), and (0,10,0). Next we connect the keypoints using straight lines and arcs, Fig 1.
The next step is to create the area using the four lines/arcs. The area can then be extruded in the z-direction to create the volume. We extrude the area in the +z direction making the disk 1.0 units wide. The final volume is shown in Fig 2.
The first analysis will be the heat transfer, so we set the element type to Solid87 and create a volume mesh. We first divide the lines (as seen in Figure 1) to guide the meshing. From the Meshing menu, select Size Cntrls and then select ManualSize. Divide the long edges and arcs into 15, the short arcs into 6, and the short edges in the z-direction into 2 segments. Select Mesh from the Meshing menu, and then select Volume and Free. Pick the volume. It will be meshed with tetrahedral elements, Fig 3.
The next step is to apply boundary conditions. This consists of temperatures on two surfaces. We make the temperature at the inner radius of the disk 1000 and the temperature at the outer radius is 100. From the Loads menu, select Define Loads, then Apply, then Thermal, then Temperature on Areas. Choose the surface at the inner radius and select OK and choose TEMP from the list of degrees of freedom and set the value to 1000. Do the same for the outer radius using a value of 100. Fig 4 shows the resulting boundary conditions that are transferred to the mesh.
Perform the solution, choosing Solution and Solve and Current LS. The analysis should take a few seconds. Proceed to the General PostProc(essing) menu, and choose Plot Results, Contour Plot, and Nodal Solution. Choose Nodal Temperature from the DOF Solution listing. The nodal temperatures should appear as in Figure 5.
The next step is to apply these temperatures to the disk model as initial conditions for the structural analysis. We can list the nodal temperatures to a file for now. We can have ANSYS apply the temperatures to the model, using the Loads, Apply, Initial Conditions, Temp from ANSYS menu option.