# Experimental and Numerical Studies of Vertical Stresses
## 3 Finite Element Analysis  
The analysis of the vertical stress values beneath the centerline of the circular footings resting on the sand bed was carried out using the commercially available computer program ANSYS (version 10), which solves with the finite element method. ANSYS is a finite element modeling package program developed to analyze various engineering problems numerically. The ANSYS program allows for effective studies in different disciplines such as mechanics, linear or non-linear static, and dynamic structural analysis. Within the scope of this study, two- and three-dimensional finite element analyses were carried out in order to support the results of the experimental study and to determine the vertical stress distribution in the sand bed subjected to load transferred from circular footing. Two different models were used for the analyses: the 2D axisymmetric model (2 DM) and the 3D model (3 DM) with the same dimensions as the model tests setup used in the experimental study. In the numerical study, the aim was to analyze the effects of 2D and 3D conditions on vertical stress values by analyzing the test setup with 2D axial symmetry and 3D modeling. By using the axisymmetric model in analysis, modeling and analysis time can be greatly reduced compared to an equivalent 3 DM. There are material models such as Mohr-Coulomb, Von Mises, and Drucker-Prager for modeling the soil material numerically. These include the elastic and plastic model parameters such as E (elasticity modulus), \(\mu\) (Poisson's ratio), cohesion c, internal friction angle \(\O\), and dilatation angle, \(\psi\). Among the mentioned methods, the Drucker-Prager criterion is frequently used in numerical analysis as one of the most suitable in terms of numerical efficiency. In this study, the Drucker-Prager elastoplastic criteria has been used to model sand behavior. The Drucker-Prager material model in the ANSYS program, the required parameters of elasticity modulus, Poisson's ratio, and shear strength of the sand were obtained by laboratory experiments performed on the samples taken from the sand in accordance with ASTM D7181-20 [27], and they are presented in Table 2.  
In the analyses, SOLID45 element type was used for the three-dimensional modeling of the soil-footing system (Figure 5). SOLID45 element type is defined by eight nodes with three degrees of freedom in the x, y, and z directions at each node. The element has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities. PLANE42 element type is used to model the soil-footing system in 2D modeling (Figure 6). The element is suitable for two-dimensional modeling, axial-symmetrical and plane-strain conditions. PLANE42 element type is defined by four nodes having two degrees of freedom in the nodal x and y directions at each node. The PLANE42 element type, similar to the SOLID45 element type, has the capabilities of plasticity, creep, swelling, stress hardening, large deflection, and large strain. In the numerical study, mesh analyses were performed on the model in order to determine the effects of mesh geometry on the results. In the mesh analysis, it was seen that the geometry of the mesh can affect the vertical stress distribution in the sand beneath the \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Parameters** & **Symbol** & **Unit** & **Value** \\ \hline Elasticity modulus & E & kN/m\({}^{2}\) & 28,000 \\ Poisson’s ratio & \(\mu\) & - & 0.20 \\ Cohesion & c & kN/m\({}^{2}\) & 0.10 \\ Internal friction angle & \(\Theta\) & (\({}^{\circ}\)) & 41 \\ Dilatation angle & \(\psi\) & (\({}^{\circ}\)) & 11 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Parameters of DP model. Figure 5: SOLID45 geometry. Figure 6: PLANE42 geometry. circular footing. As a result of the analyses, a mesh geometry with the medium mesh option that does not affect the vertical stress distribution was selected, and this mesh geometry was used in the subsequent analyses.