## 3 Numerical Modelling of the Dapped-End Beam  
To perform a parametric analysis on a dapped-end beam and to examine the influence of the prestressing force, a numerical model was developed utilizing the finite element analysis software DIANA FEA. The drawings of the models are shown in Figures 5 and 6. The width of the beam \(b=200\) mm, the length \(L=3000\) mm, and the height \(H=600\) mm. The beam was modeled as a 3D solid element, which can be observed in Figure 7. The beam model was supported by simulated plates with dimensions of 100 mm in length, 200 mm in width, and 40 mm in height. An identical plate was used to apply loads. The plates were modelled as 3D solid elements. The displacement of the left support was constrained in all directions and constrained in rotation around the z and x axes. The right support was equivalent to the left, but the displacement was not fixed along the x-axis. The model of the beam was exposed to two loads: a load of its own weight and an external load on the load plate. Between the surface of the plates and their imprint on the beam, a 3D surface interface was modelled. For the plate steel, an elastic material model was selected with a modulus of \(E=210\) GPa, a Poisson's coefficient of \(v=0.3\), and a density of \(\rho=7850\) kg/m\({}^{3}\). Figure 5: _Cont._  
Figure 5: Drawings of the non-prestressed beam model: (**a**) drawing of the specimen; (**b**) geometry and reinforcement arrangement of the dapped end. Figure 6: Drawings of the prestressed beam model: (**a**) drawing of the specimen; (**b**) geometry and reinforcement arrangement of the dapped end. Figure 7: Numerical model of the dapped-end beam: (**a**) 3D model of the beam; (**b**) Meshed 3D elements; (**c**) Reinforcement model. The finite element (FE) mesh was composed of elements of varying sizes (see Figure 7b) not only to achieve the required accuracy of the calculations but also to maintain a rational duration of computer calculation. The beam was divided into several zones where the FE sizes differ: the zone around the left end of the beam was divided into square elements \(20\times 20\times 20\) mm in size, the re-entrant corner of the notch was divided into elements \(10\times 10\times 10\) mm in size, and the wall of the right notch was divided into \(20\times 20\times 20\) mm-sized elements (to more accurately assess the deformations caused by the prestressed reinforcement). The rest of the beam model was divided into 50 mm adaptive dimensional-size FEs. The size of the FE of the support and load plates was chosen to form at least two FEs through the thickness of the plates. In the numerical model, concrete was defined as an elastic-plastic material. A total train-based crack model was selected for the concrete model. The behavior of concrete under compression was defined by a parabolic stress-strain relationship curve (see Figure 8a) and the tensile behavior was defined by an exponential curve (see Figure 8b). The material properties employed in this research were derived from the study conducted by [PERSON] et al., 2003 [PERSON] et al. (2003). The remaining concrete parameters were selected according to EN 1992-1-1 Table 3.1 [7]. Based on an average compressive concrete strength of 33.7 MPa, the C25/30 concrete class was chosen. The following parameters were adopted: concrete modulus of elasticity \(E_{cm}=31.675\) GPa; tensile strength \(f_{cm}=2.613\) MPa; Poisson's ratio \(\
u=0.2\); concrete density \(\rho=2400\) kg/m\({}^{3}\). The specified concrete model in the numerical model necessitated certain concrete properties that were not provided in the table. These parameters were estimated using the subsequent formulas. The dependence between compressive concrete strength and fracture energy when concrete is under compression can be expressed through the following formula [23]:  
\[G_{c}=15+0.43\cdot f_{cm}-0.0036\cdot f_{cm}^{2}, \tag{13}\]  
where \(f_{cm}\) is the average compressive strength of concrete in MPa; \(G_{c}\) is fracture energy under compression in N/mm.