PSI - Issue 52

Leonardo Gunawan et al. / Procedia Structural Integrity 52 (2024) 560–569 Author name / Structural Integrity Procedia 00 (2019) 000 – 000

563

4

3. FEM Model Numerical simulations were performed using ABAQUS CAE software with the Coupled Eulerian Lagrangian (CEL) method that combines the Lagrangian framework and the Eulerian skeleton, commonly used to analyze the interaction between solid body (Lagrangian) and fluid (Eulerian) (Abaqus User Guide, 2014). Simulation using this method requires high computational resources because it uses 2 frameworks at once (Muharram, 2009). The model consisted of a hollow box and the water in the vessel. The hollow box model was divided into 3 parts as described earlier, namely the base frame, the side panel, and the base panel. 3.1. Hollow Box The base frame was in the form of a solid square box with a square hole in the middle with an outer size of 400 mm × 400 mm, an inner size of 320 mm × 320 mm, and a height of 40 mm. The mesh type of this section was 3D linear solid elements with reduced integration point (C3D8R) with a global mesh size of 10 mm as shown in Fig.3.a. Each of the 4 side walls is 400 mm wide, 500 mm high, and 0.3 mm thick and were connected by 4 corner plates with a length of 550 mm, a flange width of 50 mm and a thickness of 0.3 mm. Physically, the walls and corner plates were joined using nuts and bolts, they were considered as an integrated component without nuts and bolts in the model. The sidewalls were modeled using a 3D conventional shell (S8R) mesh type with a global mesh size of 10 mm as shown in Fig.3.b. The side walls and the base frame were not parts that failed, so the mesh sizes for these two parts did not need to be too small.

Fig. 3. a. Base frame. b. Side panel. The base panel is in the form of a 400 mm × 400 mm square plate with thickness of 0.3 mm. In the center of the base panel, a small hole with a diameter of 5 mm is made. The hole is intentionally located to serve as a stress raiser to promote damage and crack emanating from it. In addition to the hole, four cross slits around the hole were added with initial length of 2.5 mm, referred here as the initial cross-cut. The purpose of the initial cross-cut is to allow failure to occur when subjected to impact loads. Such zero thickness slits (or cross cut) was made by using the so called seam feature in Abaqus as shown Fig. 4. Around the cross-cut, the plate was discretized with 3D shell elements (S8R) with a global mesh size of 2.5 mm. This was done following the model developed by Francescino (2009) and convergence tests showed that failures that occurred with a mesh size of 2.5 mm were the same as failures that occurred using a mesh measuring 1.25 mm. In this study, the box models were simulated with two different strategies to connect the base plate with the frame. In the first model (Model 1), the base plate was clamped perfectly to the base frame on all four sides with Abaqus *TIE constraint. This was done following the referred work to simplify bolts mounted on base panels and base frames. The part of the base panel that attaches to the base frame is designated as the slave surface because it is the part that is more likely to fail and has a smaller mesh. The given part of the tie constraint can be seen in Fig. 4(a). The entire