## 2 Materials and Methods
### Numerical Analysis  
The 3D representation of the unit cells used for numerical modelling and analysis are demonstrated in Figure 5. The actual FE models of the unit cells along with the boundary conditions are demonstrated in Appendix D. The struts of the unit cells were discretized using Timoshenko beam elements (element type BEAM189 in ANSYS), and each strut was discretized using five beam elements. The beam elements were rigidly connected to each other at their shared vertices, and they were not allowed to rotate in any direction at the connecting point. The mechanical properties of the titanium alloy Ti-6 Al-4V-ELI were used for modelling the behaviour of the matrix material in the FE models. A linear elastic material model with elastic modulus and Poisson's ratio of 113.8 GPa and 0.342, respectively, was implemented. Since the BEAM189 element uses linear interpolation and takes transverse shear deformation into account, it is expected that the numerical results will be closer to the Timoshenko analytical solution. In the FE models of BCC, diamond, truncated cube, and truncated octahedron, a single unit cell with periodic boundary condition was analysed under compressive loading (Figure A2a,b,e,f in Appendix D). For the hexagonal packing and rhombicuboctahedron topologies, lattice structures consisting of 11 \(\times\) 11 \(\times\) 11 unit cells were used for numerical modelling. This was due to the complexity of modelling the repetitive boundary conditions in these two unit cell types. More specifically, in these two cases, each side of the unit cell is composed of two strut types (rather than one strut type in the case of other unit cell types), which have non-symmetrical displacements under compressive loading (demonstrated as strut types A and B in Figure 5c,d). In all the FE models, the lowermost nodes of the structure were fixed in the direction parallel to the loading direction and were not allowed to rotate in any direction. For the case of FE models made out of single unit cells (Figure A2a,b,e,f in Appendix D), the side vertices of the unit cell were constrained rotationally as they were symmetrically connected to the (imaginary) adjacent unit cells (repetitive boundary condition). In all the FE models, a downward displacement was applied on the uppermost node(s) of the structure to induce axial deformation. Moreover, the uppermost nodes were not allowed to rotate in any directions. Mechanical properties of the FE models have been calculated based on the basic definition of elastic modulus, Poisson's ratio, and yield stress:  
* Elastic modulus: The formula \(E_{UC}=\frac{F_{UC}L_{UC}}{A_{UC}\omega_{UC}}\) was used for calculating numerical elastic modulus, where \(L_{UC}\) is the structure length in the direction parallel to loading direction, \(A_{UC}\) is the cross-sectional area of the structure in the direction perpendicular to the loading direction, \(\delta_{UC}\) is the downward displacement applied to the uppermost nodes, and \(F_{UC}\) is obtained by summing the reaction forces of the lowermost nodes. * Poisson's ratio: The formula \(\upsilon_{UC}=-\frac{\epsilon_{2}}{\epsilon_{1}}=-\frac{L_{1}\delta_{2}}{L_{2 }\delta_{1}}\) was used for obtaining Poisson's ratio. In this formula, \(\delta_{1}\) and \(L_{1}\) are the downward displacement applied to the uppermost nodes and unit cell's length in the direction parallel to loading direction, respectively. Parameters \(\delta_{2}\) and \(L_{2}\) are respectively the lateral displacement of the side nodes and the structure length in the direction perpendicular to loading direction. * Yield stress: The formula \(\frac{\sigma_{y}}{\delta_{yz}}=\frac{F_{UC}}{A_{UC}\omega_{max}}\) was used to calculate normalized yield stress. In this formula, \(\sigma_{max}\) is the maximum von Mises stress experienced in the most critical point of the structure. The critical points of each unit cell can be seen in Section 4.1.