FEM for Two-Dimensional Solids (Finite Element Method) Part 5

Solution Process

Let us now try to relate the information we provided in the input file with what is covered in this topic. As before, the first sets of data usually defined are the nodes and their coordinates. Then, there are the element cards containing the connectivity information. The importance of this information has already been mentioned in previous case studies. Looking at Figure 7.23, it is not difficult to guess that the element used is an isoparametric quadrilateral element (CPS4-2D, quadrilateral, bilinear, plane stress elements), rather than that of a rectangular element. Obviously, it can be visualized that using rectangular elements would pose a problem in meshing the geometry here. In fact, the use of purely rectangular elements is so rare that most software (including ABAQUS) only provides the more versatile quadrilateral element. This information from the nodal and element cards will be used for constructing the element matrices (Eqs. (7.80) and (7.81)).

Next, the property cards define the properties of the elements, and also specify the material the elements should possess. For the plane stress elements, the thickness of the elements must be specified (13 ^m in this case), since it is required in the stiffness and mass matrices (the mass matrix is actually not required in this case study, since this is a static analysis). Similarly, the elastic properties of the polysilicon material defined in the material card are also required in the element matrices. It should be noted that in ABAQUS, the integral in Eq. (7.80) is evaluated using the Gauss integration scheme, and the default number of Gauss points for the bilinear element is 4.

The boundary cards (BC cards) define the boundary conditions for the model. To model the symmetrical boundary conditions, at the lines of symmetry (x = 0 and y = 0), the nodal displacement component normal to the line is constrained to zero. The nodes (node set, FIXED) along the centre hole where the hub should be is also fully clamped in. The load cards defined specify the distributed loading on the motor, as shown in Figure 7.23. These will be used to form the force vector, which is similar in form to that of Eq. (7.64).

The control cards are used to control the analysis, which in this case defines that this is a static analysis. Finally, the output cards define the necessary output requested, which here are the displacement components, the stress components and the strain components.

Once the input file has been created, one can then invoke ABAQUS to execute the analysis, and the results will be written into an output file that can be read by the postprocessor.

Results and Discussion

Using the above ABAQUS input file that describes the problem, a static analysis is carried out. Figure 7.24 shows the Von Mises stress distribution obtained with 24 bilinear quadrilateral elements. It should be noted here that 24 elements (41 nodes) for such a problem may not be sufficient for accurate results. Analyses with a denser mesh (129 nodes and 185 nodes) using the same element type are also carried out. Their input files will be similar to that shown, but with more nodes and elements.

Figure 7.24. Analysis no. 1: Von Mises stress distribution using 24 bilinear quadrilateral elements.

Figure 7.25. Analysis no. 2: Von Mises stress distribution using 96 bilinear quadrilateral elements.

Figures 7.25 and 7.26 show the Von Mises stress distribution obtained using 96 (129 nodes) and 144 elements (185 nodes), respectively. Figure 7.27 also shows the results obtained when 24 eight-nodal elements (105 nodes in total) are used instead of four-nodal elements. The element type in ABAQUS for eight nodal, plane stress, quadratic element is ‘CPS8’. Finally, linear, triangular elements (CPS3) are also used for comparison, and the stress distribution obtained is shown in Figure 7.28.

From the results obtained, it can be noted that analysis 1, which uses 24 bilinear elements, does not seem as accurate as the other three. Table 7.3 shows the maximum Von Mises stress for the five analyses. It can be seen that the maximum Von Mises stress using just 24 bilinear, quadrilateral elements (41 nodes) is just about 0.0139 GPa, which is a bit low when compared with the other analyses. The other analyses, especially from analyses 2 to 4 using quadrilateral elements, obtained results that are quite close to one another when we compare the maximum Von Mises stress. We can conclude that using just 24 bilinear, quadrilateral elements is definitely not sufficient in this case. The comparison also shows that using quadratic elements (eight-nodal) with a total of 105 nodes, yielded results that are close to analysis 3 with the bilinear elements and 105 nodes. In this case, the quadratic elements also have curved edges, instead of straight edges and this would define the curved geometry better. Looking at the maximum Von Mises stress obtained using triangular elements in analysis 5, we can see that, despite having the same number of nodes as in analysis 2, the results obtained showed some deviation. This clearly shows that quadrilateral elements in general provide better accuracy than triangular elements. However, it is still convenient to use triangular elements to mesh complex geometry containing sharp corners.

Figure 7.26. Analysis no. 3: Von Mises stress distribution using 144 bilinear quadrilateral elements.

Figure 7.27. Analysis no. 4: Von Mises stress distribution using 24 eight-nodal, quadratic elements.

Figure 7.28. Analysis no. 5: Von Mises stress distribution using 192 three-nodal, triangular elements.

Table 7.3. Maximum Von Mises stress

From the stress distribution, it can generally be seen that there is stress concentration at the corners of the rotor structure, as expected. Therefore, if structural failure is to occur, it would be at these areas of stress concentration.