# Two-Dimensional Mesoscale Finite Element Modeling of Concrete Damage and Failure
## 3 Automatic Generation of Cohesive Elements
The final simulation results are obtained by calculating the average of these ten individual simulations, ensuring a representative and reliable outcome for the study. Figure 5: Fracture criterion and boundary conditions. (**a**) Mixed-mode B-K fracture criterion. (**b**) Applied boundary conditions in mesoscale simulations. Incorporating the cohesive zone model (CZM) for concrete materials consists of two crucial steps. Initially, concrete mesostructure creation occurs through algorithms specified in Section 2, followed by model discretization. Afterwards, the model's input file is integrated into CZM algorithms to generate cohesive elements. Although CZM proficiently depicts concrete's complex behavior under varied boundary conditions, it is limited by model mesh dependency. Using smaller elements can mitigate this, yet it elevates computational cost due to an increased element count. Thus, a mesh sensitivity analysis is essential to strike a balance between computational efficiency and model accuracy. ### Model Parameters

Three-node triangular elements (CPS3) are used to discretize the entire 2D mesoscale finite element model (see Figure 6). The cohesive zone model is mesh dependent, and during the calibration process it was found that a mesh size of 1 mm can provide a good compromise between the computational cost and a reduction in the mesh sensitivity problem. The B-K fracture criterion with quadratic nominal stress criterion and linear softening law was utilized to model the material behavior of the cohesive elements. Ten mesoscale samples, each featuring unique spatial distributions of aggregate particles, undergo multiple simulations using varied input parameters of the TSL for cohesive interface elements (CIEs). The simulation results, including stress-strain curves, are obtained by averaging the outcomes of these simulations. The stress for each stress-strain curve is determined by summing the nodal reaction forces in the constrained edge and then dividing the sum by the length of the specimen at each step frame. These stress-strain curves are then compared with experimental data. Through this comparative analysis, the input parameters of the TSL for CIEs are calibrated for mesoscale simulations. The calibrated TSL properties for different phases are listed in Table 2. A mesh size of 0.5 mm is deliberately chosen for the calibration process to mitigate, as much as possible, the mesh dependency. This discretization level results in a total of 87,000 solid elements and 130,000 CIEs. Notably, some material properties of the mortar matrix and aggregates particles are obtained from [32; 46]. For the uniaxial tensile simulations, the nodes at the left boundary are constrained in the x-direction, while those at the right boundary are displaced by 0.15 mm. The applied boundary conditions are depicted in Figure 5b. To handle model nonlinearity and convergence challenges, the explicit Abaqus solver is utilized with a step time of \(4\times 10^{-7}\), ensuring quasi-static loading conditions. Figure 6: The concrete sample has been discretized using a finite element method with a mesh size of 1 mm. To provide a clearer view of the mesh configuration, the elements within the red box have been magnified. ### Mesh Convergence Study

For finite element simulations where the cohesive crack paths are not known in advance, rather fine levels of discretization must be used to reduce the dependence of the cohesive crack paths on the mesh size. However, reducing the element size leads to an increase in computational cost, so a balance between computational cost and accuracy must be established. To this end, a mesh convergence study is performed in this work in terms of the mean stress-strain curve and the final fracture crack paths to find an optimal mesh size. In this work, a mesoscale specimen with circular aggregates and volume fraction of 50% is discretized with six different discretization levels. After discretization, all specimens are subjected to a uniaxial tensile test simulation.