# Analysis of a Preliminary Design Approach for Conformal Lattice Structures
## 2 Materials and Methods
### Beam Approach for Linear Structural Analysis  
In this section, the implemented beam structural linear analysis approaches are presented. The FEM analyses were performed to validate the optimized lattice structure models. Three displacement-based FEM software were employed:  
* Karamba3D (1.3.3) plug-in with Rhinoceros 7 (7.8.2) [54]. Karamba3D is a parametric structural engineering tool that performs structural analyses of spatial trusses, frames, and shells, and it is fully embedded in the parametric environment of Grasshopper, the visual programming language inside Rhinoceros. This makes it easy to combine parameterized geometric models, finite element analyses, and optimization algorithms. Karamba3D has been mostly used in the early stage design [65];
* MSC Patran/Nastran [47]. Patran is a pre-/post-processing software for FEA that provides modeling, meshing, analysis setup, and post processing for solvers. Nastran is a multidisciplinary structural solver for accurate static, dynamic, and thermal analyses;
* Ansys 2020 R1 Mechanical [44]. Ansys is an FEA software tool for multidisciplinary simulation with a common platform, ANSYS Workbench, that can connect the tools together. As for Nastran, ANSYS Mechanical is the dedicated tool for multidisciplinary structural analyses. In Karamba3D, the structural beam analysis is based on the Timoshenko beam theory with a linear shape function [65]. In Nastran, the beam model is based on the Euler-Bernoulli beam element. In ANSYS Mechanical, two types of the beam element can be selected: _beam 188_ (or _beam 189_) based on the Timoshenko theory and _beam 3_ based on the Euler-Bernoulli theory; moreover, through the Mechanical APDL interface, it is possible to select the type of the shape function (linear, quadratic, cubic) to define more integration points along with the element for enhancing the results and visualization accuracy; in this work, the _beam 188_ element with a quadratic shape function was selected. In the Euler-Bernoulli beam theory, it is assumed that the plane cross-sections remain plain and perpendicular to the axis of the beam after the deformation; this assumption involves that all the transverse shear strains are null. The [PERSON] beam theory is an extension of the Euler-Bernoulli one: the plane of the sections remains plain but not necessarily perpendicular to the longitudinal axis after the deformation, thus admitting a nonzero transverse shear strain [66]. In operational terms, for a static case, [PERSON]'s beam model, if compared to [PERSON]'s model, has an additional energetic contribution given by the shear. A number of refined theories have been proposed for the analysis of shear deformable beams in the last four decades [67; 68; 69; 70; 71; 72], but they are not adopted by \begin{table}
\begin{tabular}{c c} \hline \hline Density & 2700 Kg/m\({}^{3}\) \\ Young modulus & 68 GPa \\ Yield strength & 190 MPa \\ Ultimate tensile strength & 335 MPa \\ Poisson ratio & 0.30 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Material properties of ASi10 Mg produced by SLM technology [63]. Figure 4: Boundary condition of the traction load case: (**a**) Karamba3D, (**b**) Nastran, and (**c**) ANSYS Mechanical. the used commercial FEM software and are beyond the scope of this work. Regardless of the software, a simplification of the geometry is mandatory since the conformal cells are described by curves, whereas the application of the beam theories requires lines. To do this, the start and the end of each transformed element are connected by a line. The beam structural validation using Karamba3D is carried out in the same environment of the NURBS-FFD modeling approach and the size optimization, so the information about the structure, material, and boundary conditions are directly available and easy to modify. Patran/Nastran and Ansys software require instead to import the model information through text files and to develop ad-hoc scripts using the dedicated programming languages of the FEM software.