Issue 63

M. Khalaf et alii, Frattura ed Integrità Strutturale, 63 (2023) 206-233; DOI: 10.3221/IGF-ESIS.63.17

CFRP sheets are classified into two types as unidirectional and bidirectional according to their orientation. The unidirectional CFRP sheets are used in current study since they behaves as a typically linear elastic material up to failure stage and does not display any yielding behavior as does the conventional reinforcing steel. The used CFRP sheets have a thickness of 0.13mm, a density of 1.82g/cm 3 , an elongation at break of 1.5%, and an ultimate tensile strength of 3500 MPa . The parameters used to identify the properties of CFRP sheets in ANSYS standard are the modulus of elasticity in the x direction (E x = 230000 MPa ), the Poisson’s ratio in the y-z plane (  yz = 0.3), the Poisson’s ratios in xy and xz-planes (  xy =  xz = 0.22), the shear modulus in the xy and xz planes (G xy =G xz =11790 MPa ) and the shear modulus in the yz plane (G yz = 6880 MPa ) [10]. Referring to Figs. 4-a and 4- b, the current research considers the layered structural solid SOLID185 and theSOLID65 elements as the finite elements types used to model the CFRP sheets and the epoxy resin layer respectively.

N UMERICAL NON - LINEAR MODELING TECHNIQUE VERIFICATION

T

he validation of the currently adopted RC beams and their proposed strengthening technique finite element modeling details according to the ANSYS software standard [26] is now detected to decide its reliability to perform the current planned research program guided by the available previous achieved experimental work results by Abdalla et al. [6].

Figure 5: The previous achieved experimental work details which considered as the numerical verification reference [6].

First of all, the nonlinearity in ANSYS software is according to the nonlinear structural behavior which is simulated by a number of factors and it can be categorized into "material nonlinearity" and "geometric nonlinearity". The nonlinear material behavior is caused by the change in the stiffness during the different loading stages while the large deformations caused the change of the geometric configurations of the structure which leads to the nonlinear response of the structure. The "Newton-Raphson" approach is employed by ANSYS for solving the nonlinear problems. In this approach, the applied total load is subdivided into a group of load increments known as load steps. The load increments are applied over a number of the load sub steps. The load applied to the model should be increased gradually to avoid non convergence of the solution. The stiffness matrix of the model is modified to reflect the nonlinear changes in the stiffness of the structure at the end of each load increment before performing the next load increment [26]. The structural solution requires identifying: the type of the analysis (which is a structural type in the current intended study) and the analysis technique (small static displacement). The Newton-Raphson equilibrium iterations are applied in ANSYS for updating the stiffness

213