PSI - Issue 6

R.V. Fedorenko et al. / Procedia Structural Integrity 6 (2017) 244–251

249

Fedorenko R. et al. / StructuralIntegrity Procedia 00 (2017) 000 – 000

6

a)

Finite element model of the Airbus A380

b) Comparison of numerical and analytical (Riera) solutions

Fig. 5 In the calculation it was taken into account that aircraft fuselage is made of the aircraft quality aluminum alloy ALCOA 7075 while the turbine shafts are made of steel. In order to consider real mass and inertia distribution ABAQUS system “Non - structural mass” technology [5] was used. Results of ex plicit finite element modelling of aircraft impact into the rigid wall were compared with simplified analytical Riera method. An aircraft velocity at the moment of contact with rigid wall was 110 m/s. During the calculation the value of total reaction force was controlled. Figure 5 (b) shows comparison of numerical and analytical solutions. As it can be seen from figure, there is good agreement betweenvalues of reaction forces derived from the full scale finite element aircraft model and the Riera solution. However, there are some variations in the force reaction as function of the time. The first extreme point of the blue line corresponds to the moment of the airplane wing contact with the wall, the second – to the moment of the aircraft engine impact. 4.2. Finite element model of the NPP reactor building Geometrical and finite element models of campus, that includes NPP reactor structure and nearby structures, were created. Figure 6 (a) shows the geometrical model of the campus in section. Finite element model of the campus consists of three structures – reactor building, safety building steam cell. The safety building and steam cell models are made with shell elements with linear-elastic material model with properties, which are equivalent to concrete B40 material properties. The finite element model of the reactor building includes three parts, which have bonded contact between each other (Fig. 6 (b)). The detailed mesh (element size equals 0.2 m) is made on the part of the reactor structure outer containment and on the part of the defence structures of the dome. It was assumed that these parts would have maximum strains during the aircraft impact. Less detailed mesh (element size equals 1 m) is made on the parts of outer containment, where minimum strains were expected during the impact.

b

a

Fig. 6.(a) in section view of the geometrical model; (b) finite element model of the reactor structure.

Geometrical and finite models were created with dimension parameterization. Thus it became possible to vary some dimensions automatically, for example, containment vessel wall thickness or expansion angle of the “detailed” part of structure. It may be possible to vary all geometrical dimensions of the structure. The computational model utilizes linear and nonlinear concrete models (CDP and Drucker-Prager), which are used for rough and detailed parts of the reactor structure model consequently. In finite elements of the outer containment explicit reinforcement was modeled using ABAQUS “embedded elements” technology. Reinf orcement was assumed to be elastic-plastic material with properties which are equivalent to reinforcement steel A400.