## 2 Materials and Methods
### Finite Element Model and Optimization Setup  
#### 2.3.1 The Finite Element Model Setup  
The explicit FEA solver Altair RADIOSS version 2021.2 [27] is used for the simulation series. Altair's FEA preprocessor HyperMesh [28] is used to prepare and set up the models. A stationary rigid steel plate below the lattice cube acts as a foundation with a second rigid plate compressing it at a constant speed of 1000 mm/s from the top, as depicted in Figure 6. The velocity was chosen such that no inertial effects occur in the model, while the computation completes quickly enough for an acceptable total duration when executed several hundred times during the optimization. The moving plate does not have any rotational degrees of freedom and is restricted to move only on the vertical axis. The cube is compressed by 25 mm (or 50%) during a run time of 25 milliseconds. The minimum time step is limited to 0.15 microseconds to keep mass scaling significantly below 1%. Contact between beam elements is realised with a TYPE11 line contact, whereas contact between the rigid plates and the lattice body is set up with a TYPE7 general penalty contact. The latter has a constant gap factor such that the plates always touch the lattice body in an identical fashion independently of the beam element thickness. To avoid any artificial movement restrictions from the cube, no additional boundary conditions are imposed on it. Coulomb friction is applied between all parts with the friction coefficients listed in Section 2.2. The moving plate's reaction force is traced at 20 kHz to accurately assess SEA performance during the optimization runs.  
The lattice geometry is represented by 1D beam elements since this enables the easy manipulation of their thickness properties, a requirement for the proposed thickness grading method. Each strut of the lattice is split into 10 beam elements (see detail in Figure 7), ensuring that buckling can be captured adequately. Full geometric nonlinearities are considered; integrated beam elements (P18_INT_BEAM) with a circular cross-section and four integration points per section are utilized. An isotropic piecewise linear elastic-plastic material law (LAW36) is applied to model the nonlinear material behaviour. Strain rate effects are not considered since only data at one single strain rate are available to the authors.  
By default, the piecewise linear elastic-plastic law extrapolates the stress-strain curve linearly beyond the given strain range, which can result in overly stiff geometry in the post-failure strain region. Therefore, an alternative approach must be found. In Altair RADIOSS, material failure in integrated beam elements can be considered by applying a simple element deletion method when the first principal strain in an element's integration point reaches the material's failure strain. However, this results in severely underpredicted  
Figure 6: FEA model setup showing the Simple Cubic (**a**) and Isotruss (**b**) lattice structures discretized with 1D elements between the two steel plates. The lower plate is stationary and rigidly fixed, while the top plate moves downwards at 1000 mm/s for 25 ms.  
reaction forces and is, therefore, not used. An alternative to this would be a gradual, linear stress reduction to zero in elements exceeding the failure strain, but RADIOSS' implementation for integrated beam elements is faulty and not in a functioning state. Other failure models for beam elements are not available in RADIOSS. A different approach must be considered, which is why the stress-strain curve was continued at the ultimate tensile stress level. This avoids a further reaction force increase but adds to the overall compressive energy absorption of the geometry during the simulation. This is considered to be the best compromise of the given options.