PSI - Issue 54

Isyna Izzal Muna et al. / Procedia Structural Integrity 54 (2024) 437–445 Isyna Izzal Muna, Magdalena Mieloszyk / Structural Integrity Procedia 00 (2019) 000 – 000

442

6

using ROM, a theoretical model by Voight. The thermal conductivity and thermal expansion of CFRP were calculated using the mathematical mixture formula by Behren and Schapery, respectively. Then the specimen model was discretized into linear quadrilateral elements with four-node, reduced integration with hourglass control, and finite membrane strains within the thermally coupled thin shell, S4RT type. The FEM model consisted of 784 finite elements and 891 nodes. 3.2. Thermal step The simulations of thermal loading at stable continuous temperature have been performed for three specimen models as representative of each thermal group: intact (without thermal loading), the stable continuous temperature at 65 ° C (HS-A), and stable continuous temperature at 145 ° C (HS-B). The samples will have two different heat transfer schemes. The first step is thermal radiation from the temperature chamber to the sample’s surface, followed by heat conduction between material layers. The heat sample module in Abaqus was used in conjunction with the heat transfer physics, and the reference temperature at the boundaries was set to 0 ° C. The initial temperature at all nodes is 20 ° C, and the bottom face has a constant temperature of 20 ° C throughout the simulation. The sample model’s boundary conditions are determined by how it interacts with its external surroundings in order to accurately represent the physical phenomena of the experimental setup, which may insulate the edges. The heat was applied to the laminate’s top surface and is distributed from the top layer (layer 1) to the bottom layer (layer 4) with the Stefan Boltzmann constant = 5.67 x 10-8 W/m 2 K 4 and emissivity ε = 0.96. Furthermore, the sample orientation was aligned with the global axis, which identifies the different faces of the laminate. The specimen model and its boundary conditions for the thermal loading are presented in Figure 4. 3.3. Mechanical step Stress analyses were performed on the developed finite element model of the composite specimen under static load. The boundary conditions and loads are applied similarly to the actual tensile test, so that the experimental work is replicated. The boundary conditions for tensile test simulation are set to be fixed (encastred) in all directions in the lower grip, and free in the direction of the applied load in the upper grip (unconstrained) in the longitudinal direction). These options ensure that the tensile test simulation is as accurate as possible, with no rotations or bending. The upper grip load was applied using surface traction, and the magnitude was calculated using the appropriate maximum force possessed by each specimen group, which was then distributed uniformly with the general traction type. The tensile test specimen model with boundary and loading condition is presented in Figure 4. When a mechanical force applied to a thin composite plate causes it to break, the structure fails relatively quickly because the load increases as the structure’s load -carrying capacity decrease. When using displacement-controlled loading, the weight of the structure decreases as it fails, allowing for a slower rate of failure.

a )

b )

Fig. 4. Boundary conditions for a) Thermal step, and b) Mechanical step.