Free Modal Stress Analysis of Electrical Machines

Introduction

The aim of this application note is to investigate the use of the Free Modal Stress solver, or Eigen Values solver (Stress EV) for machines specific applications. The modal solver allows the evaluation of the natural frequency response of structures and the identification of the resonant frequencies that could create excessive vibration if excited. This is particularly important for machines applications were variable frequency drive is common.

A high number of parameters can influence the Eigen modes identified by the analysis, both relating to the geometrical definition of the model and setup. This study will not investigate the influence of model dependent parameters, such as mechanical material properties or fixing points. The investigation will focus instead on model boundary conditions, mesh size and element type as well as the use of symmetry, in order to identify key features for machine applications.

In this example, the stator of a Switched Reluctance machine (SRM) is modelled and analysed. The free modal response of other machine components, such as rotor and shaft could also be modelled, either individually or as a complete system. If the bearings and outer casing are included, the SRM could be modelled completely.

The effect that the windings would have on the response of the entire stator structure could also be modelled; however this would require the knowledge of the mechanical parameters for the interaction between stator steel, copper and insulation. This is beyond the scope of this application note, and hence, the stator steel is modelled independently.

Model description

The stator of the modelled Switched Reluctance Machine (SRM) has six poles, with small pole tips that extend beyond the edge of the pole. The ratio of the stator length to the external diameter is approximately 1.7.

The material used for the stator and pole is considered to be isotropic with the following mechanical properties:

  • Young’s Modulus: 220 GPa
  • Poisson’s Ratio: 0.3
  • Density: 8030 kg/cm3

Note that, of course, a laminated stack is not really isotropic. Orthotropic or fully anisotropic properties may also be specified.

The frequency range for the modal stress analysis is set to [0 … 20.000] Hz and the maximum number of eigenvalues to be identified for each simulation is 100.

Figure 1: SRM stator used for stress EV analysis

Figure 1: SRM stator used for stress EV analysis

The stator is fixed on the exterior radius with four narrow strips along the entire length of the stator back-iron. A fixed boundary condition is applied onto these faces, while the rest of the structure has unrestricted movement. This setup is consistent with the techniques used for real world applications.

Figure 2: Fixing points on the exterior radius of the stator back-iron

Figure 2: Fixing points on the exterior radius of the stator back-iron

Implications of boundary conditions

A number of different model symmetry options are available for Opera-3d Stress EV models, which allow the reduction of the size of the model that needs to be evaluated. The application of the rotational symmetry option is not feasible in this case since the rotational component of the free Eigen modes is not periodic. This is because the fixing surfaces and pole numbers exhibit different symmetry. Hence, only an axial symmetry boundary condition is applied. The ‘Normal displacement fixed’ condition is used in the XY plane. This would allow solving half of the model in the axial direction, thus reducing time and computational effort. The reduced model with the applied boundary condition is shown in Figure 3. This boundary condition constrains the modes on the symmetry plane to only be allowed to move in the radial and azimuthal directions.

A full model is solved and used as a benchmark in order to establish whether the assumptions made by the application of the axial boundary condition are applicable for this type of application. The frequency range which will be investigated by the modal analysis is from 1 to 20,000 Hz.

Figure 3: XY symmetry applied (Fixed Normal boundary condition)

Figure 3: XY symmetry applied (Fixed Normal boundary condition)

The resonant modes for three of the identified frequencies are compared in Figure 4, between the full model and the half model with axial symmetry. For visualisation purposes, the complete model is displayed in the Post-Processor for both cases, with the mention that only half of the model is solved when using the symmetry boundary condition.

For these three modes, which are dominated by radial and azimuthal displacements, the frequencies at which these occur and the computed deformations are identical.

Figure 4. Comparison of resonant modes: left – full model; right – XY symmetric model

Figure 4. Comparison of resonant modes: left – full model; right – XY symmetric model

The full model has identified almost twice as many modes as the model using the XY symmetry boundary condition: 87 vs. 47 modes respectively in the 1 to 20,000 Hz range (see Figure 5). In addition to the modes existing in the XY symmetric model, the full model identified extra modes which have a predominant axial component.

Figure 5. Frequency of identified modes (full model vs. XY symmetric)

Figure 5. Frequency of identified modes (full model vs. XY symmetric)

These modes cannot be obtained by the model which uses the Fixed Normal Boundary Condition imposed on the XY symmetry plane. An example of such a mode is shown in Figure 6.

Figure 6. Axial-component-dominated mode identified from the full model

Figure 6. Axial-component-dominated mode identified from the full model

It can thus be concluded that the use of an axial symmetry boundary condition will reduce the degrees of freedom allowed in the model and consequently lead to the identification of only a sub-group of the structure’s Eigen modes and frequencies.

Implications of mesh

The implications of the mesh definition in the accuracy and solving time of modal analysis models are discussed in this section. The influence of three different parameters is considered:

  • Mesh element size – The size of mesh elements is an obvious first parameter to investigate when solving FE models. An inadequate level of discretisation can lead to less accurate results, while an over-meshed model might result in extreme solving times without any real benefit in predicting the correct results. The problem of the mesh definition can be rather different for stress analysis models, where a mesh that would be adequate for electromagnetic FE calculations might not be appropriate. Ten different levels of discretisation are looked at, starting with a very fine grained mesh, referred in the following as “mesh size=1” (shown in Figure 7.a) up to a very coarse one, referred to as “mesh size=10” (shown in Figure 7.b). The mesh sizes for the intermediate eight cases are linearly distributed between the two limits.
Figure 7. Different mesh discretisation

Figure 7. Different mesh discretisation

  • Mesh type – Opera-3d offers to the user the possibility of using tetrahedral or mosaic mesh elements. The resultant volumes can consist of all tetrahedral, all hexahedral or a combination of hexahedral, tetrahedral, prism and pyramid elements respectively. In this investigation the models are either all tetrahedral or all hexahedral meshed. From the point of view of a stress analysis, hexahedral mesh elements are less rigid compared to tetrahedral ones, which should give the hexahedral meshed models a higher accuracy at modelling deformations. The two different types of mesh used in this study are shown in Figure 8, for a mesh size of 5.
Figure 8. Different mesh types

Figure 8. Different mesh types

  • Element type – The nodal solver used in the 3d Modal EV analysis in Opera allows for either a linear interpolation of the displacement in each element or a quadratic one. The fields in quadratic elements are represented by second degree functions, giving them a higher accuracy at predicting highly non-linear results.

The influence that the first of the three parameters (mesh size) has on the results obtained from the stressEV analysis can be seen in Figure 9. The mesh type is set to tetrahedral and the element type to linear. The mesh size is varied between the limits described above and the frequencies identified by the ten cases in the range 1 to 20,000 Hz are plotted.

Figure 9. Eigen frequencies vs. modes for tetrahedral meshed model with linear elements

Figure 9. Eigen frequencies vs. modes for tetrahedral meshed model with linear elements

As it can be seen, the modes identified by the different cases are occouring at different frequencies. A further investigation into the singularity of these modes is done using only the finest and the coarsest meshed models. The shape of the deformation is checked for all the frequencies identified in the two databases in order to find the coresponding modes. In Figure 10 four of the modes that can be found in both models are shown and their shapes are presented in Figure 11.

The deformations in the case of the coarse model are the same as for the finer meshed one, suggesting that the correct modes can be identified with a coarser mesh. However, the frequencies at which these modes ocuor are significantly different. This suggests that although the major modes can be identified even with a very coarse mesh, the correct frequencies will only be identified if the mesh is sufficiently fine.

It can also be seen that the accuracy of the coarser meshed model decreases as the frequency increases, suggesting that mesh density needs to be increased when looking at the higher end of the frequency range.

Figure 10. Identified frequencies from the two extreme cases for tetrahedral mesh with linear elements

Figure 10. Identified frequencies from the two extreme cases for tetrahedral mesh with linear elements

Figure 11. Corresponding modes for tetrahedral linear mesh with different mesh size

Figure 11. Corresponding modes for tetrahedral linear mesh with different mesh size

In order to asses the influence that hexahedral mesh and quadratic elements have on the accuracy of the simulation, three more setups of the same model are run: tetrahedral mesh with quadratic elements, hexahedral mesh with linear elements and hexahedral mesh with quadratic elements,while the mesh sizes are varied in the same range as previously.

A comparison between models with the same mesh type (tetrahedral) and same mesh size (5), but different element types (linear vs. quadratic), is shown in Figure 12. Quadratic elements allow for a much better prediction of deformations using the same – or even lower – number of elements, for both tetrahedral and hexahedral mesh.

Figure 12. Deformations for tetrahedral mesh (size 5) with different element type

Figure 12. Deformations for tetrahedral mesh (size 5) with different element type

The results of these four runs (tetrahedral/ hexahedral mesh with linear/ quadratic elements) are shown in Figure 13. For ease of visualization, only the values of the two extreme cases in the mesh size range (mesh size=1 and mesh size=10) are plotted for each case.

As it can be seen, using quadratic elements instead of linear ones allows for a very accurate prediction of the Eigen modes even with a coarse mesh.

Also, switching to hexahedral elements can considerably improve the accuracy even with a coarser meshed model. Using the hexahedral mesh and quadratic elements shows the best convergence of results. However, hexahedral meshing cannot be applied to every type of geometry and may require additional model editing.

Figure 13. Mesh and element type comparison

Figure 13. Mesh and element type comparison

Solve time comparison

Alongside precision of results, the time and computation resources required by the different combinations of mesh type, size and element type need to be considered. As can be seen in Figure 14, although for the coarse meshed models the solving time between the four cases is relatively similar, there is a significant difference as the number of elements increases. Since the accuracy of the models using linear elements is consistently reliable only for the more densly meshed models, the time comparison will need to be done in this region. In the most extreme case, when the mesh is the finest, the tetrahedral linear model is around 6.6 times slower than the hexahedral meshed model with linear elements.

When comparing models using quadratic elements, the finest meshed tetrahedral model is 4.3 times slower that the equivalent meshed hexahedral model. Even more, the models using hexahedral elements do not need to be as finely meshed as tetrahedral models, hence the time difference between models with similar results would be even greater.

Figure 14. Comparison of solve time for different mesh type and sizes and element type

Figure 14. Comparison of solve time for different mesh type and sizes and element type

The time difference can be explained by the size of the solved matrix which is directly linked to the different number of degrees of freedom of the hexahedral and tetrahedral mesh. The solution matrix of the quadratic hexahedral model contains around 140.000 equations, while the matrix of the quadratic tetrahedral model contains almost 540.000 equations.

Conclusion

This application note investigates the possible variations in the setup of models for modal stress analysis, with a particular view on electrical machines applications. The use of symmetry is examined and the case is made for the necessity of the full model to be included in order to correctly capture both the radial and axial components of the deformations. In the second part, the effects that different mesh parameters have on the accuracy and speed of the solution are assessed. All possible combinations of mesh size, element type and mesh type are considered and the both the accuracy of results and solution time between the different cases are compared. Quadratic / hexahedral elements offer the most accurate results while at the same time allowing for a larger element size than in the case of tetrahedral mesh leading to faster computation times.