# Determination of the Crack Propagation Direction in Mixed-Mode Missions due to Cyclic Loading
## 3 Crack Propagation Procedure in CrackTRACER3D  
For the validation, the test results were simulated by performing cyclic crack propagation calculations using the MTU in-house software CRACKTRACER3D. This is a fully automatic cyclic crack propagation tool using the finite element method. A calculation based on CRACKTRACER3D consists of several increments. Each increment is made up of a pre-processing part, a finite element call, and a post-processing part (Figure 3). Let us for the sake of clarity at first assume that there is only one loading step. The input for the pre-processor consists of a finite element input file for the uncracked structure (including the mesh, the boundary conditions, the loading, etc.) and a file containing the actual crack geometry. The pre-processor inserts this crack into the mesh and generates a finite element deck for the cracked structure. It does so by remeshing a part of the mesh in which crack propagation is supposed to take place (the so-called domain). This domain is remeshed using quadratic hexahedral elements with reduced integration in a flexible cylinder with a hexagonal cross-section surrounding the crack front (the so-called tube) and quadratic tetrahedral elements elsewhere. All meshes were connected using linear multiple point constraints. Figure 4 shows a typical mesh during crack propagation in the tension-torsion specimen. In Part (a) of the figure, one notices the original mesh (quadratic hexahedral elements in this case) on the top and bottom. The middle part is the domain, which is primarily meshed with tetrahedral elements. At the crack front, in a hexagonal cylinder, twenty-node brick elements with reduced integration were used (Figure 5). [PERSON] [42] proved that the integration points of these elements are superconvergent, i.e., the stresses in these integration points have also a quadratic accuracy. Figure 2: Load-time curves used for the experimental investigation [38]. The innermost layer of hexahedral elements adjacent to the crack front are so-called collapsed quarter-point elements [43; 44]. These are regular 20-node brick elements, one face of which is collapsed to a line. The 8 nodes in this face are reduced to 3, i.e., one and the same node may occur more than once in the element topology. Furthermore, mid-nodes on edges having one node in common with the crack front are moved into a quarter-point position. It has been proven that these elements exhibit the \(1/\sqrt{r}\) singularity typical for the stress and strain field at the crack tip in linear elastic calculations. Figure 4: (a) Mesh of the cracked tension-torsion specimen. (b) Detail of the domain. Figure 3: Scheme of CRACKTRACER3D. After the creation of the new mesh, any boundary conditions applied to the domain were appropriately modified. Subsequently, a linear elastic finite element calculation was performed with the free software finite element tool CalculiX [45]. As a result of the calculation, the stresses at the reduced integration points in the 20-node collapsed hexahedral elements were stored in a file. The post-processor uses these stresses to obtain the K-factors (stress intensity factors) along the crack front. To this end, the stress obtained by the finite element method was compared to the asymptotic stress field at the crack front. For isotropic materials, this latter field is analytically available [46] and takes the form:  
\[\sigma_{xx}=\frac{1}{\sqrt{r}}f_{xx}(\varphi,K_{I},K_{II},K_{III}), \tag{1}\]  
and similar for the other stress components. Here, the x-y-z coordinate system is a local coordinate system at the crack front: the y-axis is locally orthogonal to the crack plane; the x-axis is in the local crack plane and locally orthogonal to the crack front in the direction of the propagation; the z-axis forms a positive coordinate system with the x and y-axis; see Figure 6. The left part of the figure gives a view of the crack plane.