Solution Process
Looking at the mesh in Figure 8.6, one can see that quadrilateral shell elements are used. Therefore, the equations for a linear, quadrilateral shell element must be formulated by ABAQUS. As before, the formulation of the element matrices would require information from the nodal cards and the element connectivity cards. The element type used here is S4, representing four nodal shell elements. There are other types of shell elements available in the ABAQUS element library.
After the nodal and element cards, next to be considered would be the property and material cards. The properties for the shell element used here must be defined, which in this case includes the material used and the thickness of the shell elements.
The boundary (BC) cards then define the boundary conditions on the model. In this problem, we would like to obtain only the flexural vibration modes of the motor, hence the components of displacements in the plane of the motor are not actually required. As mentioned, this is very much the characteristic of the plate elements. Therefore, DOFs 1, 2 and 6 corresponding to the x and y displacements, and rotation about the z axis, is constrained. The other boundary condition would be the constraining of the displacements of the nodes at the centre of the motor.
Without the need to define any external loadings, the control cards then define the type of analysis ABAQUS would carry out. ABAQUS uses the sub-space iteration scheme by default to evaluate the eigenvalues of the equation of motion. This method is a very effective method of determining a number of lowest eigenvalues and corresponding eigenvectors for a very large system of several thousand DOFs.Finally, the output control cards define the necessary output required by the analyst.
Result and Discussion
Using the input file above, an eigenvalue extraction is carried out in ABAQUS. The output is extracted from the ABAQUS results file showing the first eight natural frequencies and tabulated in Table 8.1.
Table 8.1. Natural frequencies obtained from analyses
|
Mode |
Natural frequencies (MHz) |
|
|
|
|
768 triangular elements with 480 nodes |
384 quadrilateral elements with 480 nodes |
1280 quadrilateral elements with 1472 nodes |
|
1 |
7.67 |
5.08 |
4.86 |
|
2 |
7.67 |
5.08 |
4.86 |
|
3 |
7.87 |
7.44 |
7.41 |
|
4 |
10.58 |
8.52 |
8.30 |
|
5 |
10.58 |
8.52 |
8.30 |
|
6 |
13.84 |
11.69 |
11.44 |
|
7 |
13.84 |
11.69 |
11.44 |
|
8 |
14.86 |
12.45 |
12.17 |
Figure 8.7. Mode 1.
The table also shows results obtained from using triangular elements as well as a finer mesh of quadrilateral elements. It is interesting to note that for certain modes, the eigenvalues and hence the frequencies are repetitive with the previous one. This is due to the symmetry of the circular rotor structure. For example, modes 1 and 2 have the same frequency, and looking at their corresponding mode shapes in Figures 8.7 and 8.8, respectively, one would notice that they are actually of the same shape but bending at a plane 90° from each other. As such, many consider this as one single mode. Therefore, though eight eigenmodes are extracted, it is effectively equivalent to only five eigenmodes. However, to be consistent with the result file from ABAQUS, all the modes extracted will be shown here. Figure 8.9 to 8.14 show the other mode shapes from this analysis. Remember that, since the in-plane displacements are already constrained, these modes are only the flexural modes of the rotor.
Comparing the natural frequencies obtained using 768 triangular elements with those obtained using the quadrilateral elements, one can see that the frequencies are generally higher using the triangular elements. Note that for the same number of nodes, using the quadrilateral elements requires half the number of elements. The results obtained using 384 quadrilateral elements do not differ much from those that use 1280 elements. This again shows that the triangular elements are less accurate than the quadrilateral elements. Note that the mode shapes obtained in the three analyses are the same.
Figure 8.8. Mode 2.
Figure 8.9. Mode 3.
Figure 8.10. Mode 4.
Figure 8.11. Mode 5.
Figure 8.12. Mode 6.
Figure 8.13. Mode 7.
Figure 8.14. Mode 8.
Case Study: Transient Analysis of a Micro-Motor
While analysing the micro-motor, another case study is included here to illustrate an example of a transient analysis using ABAQUS.
The rotor of the micro-motor rotates due to the electrostatic force between the rotor and the stator poles of the motor. Let us assume a hypothetical case where there is a misalignment between the rotor and the stator poles in the motor. As such, there might be other force components acting on the rotor. The actual analysis of such a problem can be very complex, so in this case study we simply analyse a very simple case of the problem with loading conditions as shown in Figure 8.15. It can be seen that symmetrical conditions are used, resulting in a quarter model. The transient response of the transverse displacement components of the various parts of the rotor is to be calculated here.
Modelling
It should be noted that an optimum number of elements (nodes) should be used for every finite element analysis. The same treatment of using the shell elements and constraining the necessary DOFs (1,2 and 6) is carried out to simulate plate elements. The difference here is that there will be loadings in the form of a sinusoidal function with respect to time,
![tmp5896-10_thumb[2]](http://what-when-how.com/wp-content/uploads/2012/06/tmp589610_thumb2.png "tmp5896-10_thumb[2]"){kind=small}
applied as concentrated loadings at the positions shown in Figure 8.15.
Figure 8.15. Quarter model of micro model with sinosoidal forces applied.
ABAQUS Input File
The ABAQUS input file for the problem described is shown below. Note that some parts are not shown due to the space available in this text.
Solution Process
The significance of the information provided in the above input file is very similar to the previous case study. Therefore, this section will highlight the differences that are mainly used for the transient analysis.
The definition of amplitude curve is important here as it enables the load (or boundary condition) to be defined as a function of time here. In this case the load will follow the sinusoidal function defined in the amplitude curve block. The sinusoidal function is defined as a periodic function whereby the formula used is actually the Fourier series. The data lines in the amplitude curve block basically define the angular frequency and the other constants in the Fourier series.
The control card specifies that the analysis is a direct integration, transient analysis. In ABAQUS, Newmarks’s method (Section 3.7.2) together with the Hilber-Hughes-Taylor operator [1978] applied on the equilibrium equations is used as the implicit solver for direct integration analysis.The algorithm used by ABAQUS is quite complex, involving the capabilities of having automatic deduction of the required time increments. Details are beyond the scope of this topic.
Result and Discussion
Upon the analysis of the problem defined by the input file above, the displacement, velocity and acceleration components throughout each individual time increment can be obtained until the final time step specified. Therefore, we have what is known as the displacementtime history, the velocity-time history and the acceleration-time history, as shown in Figures 8.16, 8.17 and 8.18, respectively. The plots show the displacement, velocity and acceleration histories of nodes 210 and 300.
Figure 8.16. Displacement-time history at nodes 210 and 300.
Figure 8.17. Velocity-time history at nodes 210 and 300.
Figure 8.18. Velocity-time history at nodes 210 and 300.
