## 4 Evaluation of Quality and Efficiency
### Optimisation of the FE Meshing  
The influence of the mesh fineness on the quality and efficiency was determined, considering:  
* Copying the results from the Gauss points to element nodes;
* The extrapolation from the Gauss points to element nodes;
* The use of additional shell elements on the surface. These are investigated on a flat specimen under axial load--see Section 4.2. The specimen consists of steel with a tensile strength of \(R_{m}=800\) MPa and a stress concentration factor of \(K_{t}=3\). When extrapolating the result variables to the element nodes, the largest errors occur with large plastic deformations. Therefore, a single load is applied with the  
Figure 16: Influence of the number of support points \(n_{M}\) of the material law on the load–notch-strain curve at different \(R_{m}\) and \(K_{t}\). high load \(L_{max,3}\) described in Section 4.2. The meshing of the specimen is conducted exclusively with hexahedron elements with a quadratic element shape function (Ansys Solid186 [71]). Other element types are also suitable for meshing the component, but these are not considered here. The user is advised to check the quality of the mesh themselves in any case in order to obtain converged stresses and strains and to exclude singularities. The meshing in the notch root is described by the number of elements \(n_{E}\) over 90\({}^{\circ}\); see Figure 17. For the elements in the notch root, edge lengths of almost the same length are used, meaning that a change in the number of elements \(n_{E}\) over 90\({}^{\circ}\) also leads to a change in the number of elements in the other directions. In addition, shell elements are added in the notch root at the component surface. In Ansys Workbench, the addition of shell elements made possible through the surface coating function [77]. Shell elements with a linear element shape function (Ansys Shell181 [78]) or with a quadratic element shape function (Ansys Shell281 [79]) are used according to the element shape function of the solid elements used. Figure 18 shows the influence of the mesh and the evaluation method used on the strain range \(\Delta\varepsilon\) and the service life at constant amplitude loading \(N_{\mathrm{const}}\). It can be observed that with increasingly finer meshing, the determined load-notch-strain curve and thus the calculated fatigue life asymptotically approach a limit value. This limit value is to serve as a reference for the evaluation of the optimizations shown below in the determination of the load-notch-strain curve. Due to the asymptotic approach to the limit value, no practice-relevant difference between the load-notch-strain curves or calculated fatigue lives can be determined above a certain mesh fineness. This mesh quality is reached at the number of elements per 90\({}^{\circ}\)\(n_{E}=70\), and will be used as a reference in the following. The influence of the meshing and the evaluation method in Figure 18A can be summarised as follows:  
* In _blue_, strain ranges are shown, which are determined by copying the result variables from the Gauss points to the element nodes. The strain ranges are underestimated, but with finer meshes, and with the associated shift of the Gauss points in the direction of the surface of the area to be analysed, they approach a constant value. This behaviour occurs both when assuming a purely elastic (_dashed line_) and an elastic-plastic (_solid line_) material behaviour. * When using the extrapolation approach (_red line_), the strain range \(\Delta\varepsilon_{\mathrm{el}}\) converges towards a fixed value with a significantly coarser mesh. In the case of elastic-plastic material behaviour, after extrapolation in Ansys Workbench, the relationship between stress and strain no longer agrees with the material law according to Equation (6). If the strain ranges from the FEA are used, the curve is almost the same as the strain ranges  
Figure 17: Meshing in the notch root of the flat specimen with \(K_{t}=3\) and \(n_{E}=30\).