## 3 Numerical Model  
The girder from Figure 1 is modelled and examined using the Abaqus FE software. Similar to the procedure described in [PERSON] et al. [21] only one quarter of the girder is modelled and adequate symmetry and boundary conditions are added (See Figure 3). Detailed information about the concrete damaged plasticity model (CDP) as used in pretensioned beams, can be found in [PERSON] et al. [21].  
Figure 3: FE model of the tested girder, prestressing strands and passive reinforcement: (**a**) Rebar and strand configuration; (**b**) End face; (**c**) Isometric view; (**d**) Lateral view.  
Figure 2: Rebar and strand configuration: (**a**) End zone; (**b**) Full beam.  
In a first step to create the geometric model in Abaqus, the geometry of the girder was implemented as mentioned in Section 2. It should be noted that at the precast plant, the positions of the vertical rebars were measured to make sure that the actual geometry is used in the FE model. At the positions of the strands, gaps are provided in the concrete girder, where in the assembly module the strands will be positioned as solid elements.  
An addition to the work of [PERSON] et al. [21] is the use of hollow strand elements. In the FEM model presented in this paper, the seven-wire strands are simplified as a hollow, cylindrical element. This allows both the strand area (139 mm\({}^{2}\)) as well as the outer diameter (15.24 mm) to be correctly implemented in the model. This avoids choosing either a correct area representation, and as such a correct longitudinal stress representation, or a correct outer surface representation, and as such a correct representation of the friction surface. When using the hollow strand element, the friction surface will be larger and smaller friction coefficients will be in agreement with the experimental results, compared to previous work, e.g., [PERSON] et al. [18] and [PERSON] et al. [21]. Finally, the small but not negligible area reduction due to the 8 seed meshing is also taken into account by means of the adaptation of the diameter of the inner circle around the hollow part. The reinforcement bars are embedded in the concrete as beam elements and the cross-sectional area of each rebar is defined in the software.  
In general, the mesh is chosen so that the computation time is not too high. Since cracks might predominantly occur at the end zones, a finer mesh is applied there. Hexahedron elements are used to increase the accuracy and automatic mesh generation is avoided. For the specific mesh generation, reference is made to [PERSON] et al. [21].  
The interaction between the strands and the surrounding concrete is defined as a surface-to-surface contact. As only a small slip occurs in the interface between the two surfaces, the \"small sliding\" option is used. Different values are used for the Coulomb friction coefficient, ranging from 0.5 to 0.9 in increments of 0.2. A hard contact has been defined, and Augmented Lagrange is used as the solver. This method uses the same approach to stiffness along the strand as the Penalty Method but allows more iterations to improve accuracy. In the tangential direction, the Penalty Method is used. The advantage is that elastic slip is also taken into account.  
In the initial step, the prestress is applied to the strands, using the predefined field function. The problem is then solved through a static analysis (Static, General), in which the prestress is applied in two stages (Initial and Step 1), see Abaqus Manual [22]. In terms of the solution method, the direct solver is applied. Compared to the iterative solver, the direct solver requires more computation time but is preferable when addressing non-linear problems. Full Newton is used as the solving technique.