## 4 Calculation
### Finite Element Simulation of the Three-Point Bending Test  
For additional evaluation of the back-calculated tensile strength values, a nonlinear finite element simulation of the three-point bending test was performed with the computer program Ansys(r) Mechanical, Release 2022 R2 [27]. Symmetry boundary conditions were applied, and only a quarter of the concrete prism was modeled. The geometry, coordinate system, loads, and support conditions can be seen in Figure 13.  
A prescribed vertical displacement (in the global Z-direction) of 3.5 mm was applied as the load (C in Figure 13) to a strip at the top of the notched cross-section with a length equal to the width of the end face of the model and with a height of 10 mm. The vertical support is marked as E (remote displacement) in Figure 13. The support E was connected to the end face of the model with a rigid element D (remote point) in Figure 13. Therefore, the displacement of the finite element model (C in Figure 13) has the same meaning as the displacement measured in the experiments, as the possible local displacement due to the support conditions is ruled out. The symmetry conditions are denoted with A and B in Figure 13. Solid finite elements of the type SOLID186 with a side length of 5 mm were used across the whole model. The SOLID186 element, a higher-order 3D 20-node solid element, displays quadratic displacement behavior and is defined by 20 nodes, each with  
Figure 13: Geometry, coordinate system, loads, and support conditions of the finite element model (**left**: view of the notched side of the model; **right**: view of the end face of the model). \begin{table}
\begin{tabular}{c c c c c c} \hline \hline
**CMOD** & **CTOD** & \(\kappa\) & \(\boldsymbol{\xi_{\text{standard}}}\) & \(\boldsymbol{\xi_{\text{calculated}}}\) & **F** \\
**[mm]** & **[mm]** & **[1/m]** & **[mm]** & **[mm]** & **[mm]** & **[kN]** \\ \hline
0 & 0 & 2.24 \(\times\) 10\({}^{-3}\) & 0.04 & 0.04 & 12.35 \\
2.09 \(\times\) 10\({}^{-2}\) & 1.74 \(\times\) 10\({}^{-2}\) & 0.0036 & 0.06 & 0.05 & 14.33 \\
0.5 & 0.42 & 0.0362 & 0.47 & 0.57 & 8.29 \\
1.5 & 1.25 & 0.1032 & 1.32 & 1.62 & 8.38 \\
2.5 & 2.08 & 0.1694 & 2.17 & 2.65 & 8.41 \\
3.5 & 2.92 & 0.2354 & 3.02 & 3.68 & 8.41 \\ \hline \hline \end{tabular}
\end{table} 
Table 8: Comparison of the calculated values (\(\xi_{\text{calculated}}\)), based on tensile strength values from expressions in the _fib Model Code for Concrete Structures 2010_[17]), and displacement values defined as per EN14651 standard [19] (\(\delta_{\text{standard}}\)) corresponding to specific CMOD values (with corresponding CTOD values, calculated curvature values (\(\kappa\)) of the notched cross-section, and load values (F)). three degrees of freedom in the nodal x-, y-, and z-directions [28]. The finite element mesh in the region of the notch can be seen in Figure 14.  
As shown in Figure 14, the notch width was equal to the mesh size (due to symmetry, only half of the notch width was modeled). The material model for the fiber-reinforced concrete was the Menetrey-Willam material model with exponential softening (see [18] for detailed information). A key motivation for using the specific material model was the relatively straightforward determination of input parameters. The Menetrey-Willam material model is the chosen material model in many studies on concrete elements (see, for example, [29]). It has also been successfully applied to steel fiber-reinforced elements (see, for example, [30]). The selected material model employs the smeared crack concept, where the mesh-dependent softening behavior is mitigated by the fracture energy model being normalized using an effective element length equal to the cube root of the integration-point volume of 3D elements.