## 3 Possibilities for the Efficient Design of FEA for the Calculation of the Load-Notch-Strain Curve
### Optimisation of the FE Meshing  
Another approach to increase the efficiency of determining the load-notch-strain curve is to optimise the meshing of the FE model. The finer the mesh in the area of the point of interest in the component is, the more accurately the stresses and strains can be determined. In contrast, the simulation time increases with finer meshing.  
By meshing the component, it is divided into discrete sections--the so-called finite elements. These finite elements consist of element nodes, which lie at the edge of the elements, and integration points, also called Gauss points, which--as a rule--lie inside the elements. The integration points are the positions in the element at which the result values determined by integration are valid. In Figure 6A, a hexahedral serendipity solid element with quadratic shape function is shown schematically. The Gauss points are marked in red and the element nodes in green. Since the result variables at the element nodes are usually of interest, these are calculated from the results at the Gauss points with interpolation or extrapolation [70]. Only this type of element (Ansys Solid 186 [71]) is used for the investigation in Sections 4 and 5 in the area of the surface to be evaluated. However, to make sure that other common element types lead to qualitatively similar results, the results are checked using the following other element types as examples:  
* Hexahedron elements with linear shape function and full integration (Ansys Solid 185 [72]);
* Tetrahedron elements with linear shape function and full integration (Ansys Solid 185 [72]);
* Tetrahedron elements with quadratic shape function and reduced integration (Ansys Solid 187 [73]).  
The exemplary investigation shows: with appropriate mesh quality, all types of elements mentioned above lead to qualitatively the same results. Fully integrated elements with a quadratic shape function, however, are not recommended due to the investigations in [74].  
This procedure is common in Ansys Workbench when using linear material behaviour, and the extrapolation provides a good estimate of the results gained at the element nodes. In the case of nonlinear material behaviour, the extrapolation of the results to the element  
Figure 6: Gauss points and element nodes: (**A**) hexahedron element (Ansys Solid186); (**B**) hexahedron element with shell element (Ansys Shell281) on one surface.  
nodes can lead to large errors [70]. These errors become larger the greater the distance between the integration point and the element node is; i.e., if the element is larger, this is also the error that occurs. Therefore, when plastic deformation occurs in the element, often no extrapolation is carried out; instead, the results gained at the integration points are copied to the element nodes [70]. This leads to an underestimation of the stresses and strains on the surface of the component and thus to an overestimation of the service life.  
The strain gradient in the notch root is relatively large in the direction vertical to the component surface. It is possible to determine the stresses and strains at the element nodes as accurately as possible if the Gauss points are as close as possible to the element nodes in the area of the component surface. On the one hand, this can be achieved by using a finer mesh at the expense of computing time. On the other hand, shell elements can be applied to the solid elements of the model at the surface of the component if only the stresses at the component's surface are of interest. Since shell elements are 2D elements, the Gauss points are on the surface; see Figure 6B. This is expected to reduce the error caused by copying or extrapolating the results and to converge the result variables to a fixed value, even when a coarser mesh is used.