Geometry and model
In this problem the joint between a pipe and a plate is analyzed. A pipe of radius 10 mm and thickness 0.75 mm is attached to a plate that is 10 mm long, 5 mm wide, and 1 mm thick. The pipe-plate intersection has a fillet radius of 1 mm. Taking advantage of the symmetry of the problem, only half the assembly is modeled. Both the pipe and the plate are assumed to be made of aluminum with E = 69 × 103 MPa, = 0.3, and = 2740 kg/m3.
The global model for the submodeling analysis is meshed with S4R elements as shown in Figure 1. The fillet radius is not taken into consideration in the shell model. The static submodel is meshed using three-dimensional C3D20R continuum elements (see Figure 2). A coarser mesh using C3D8R elements is chosen for the dynamic tests. The shell-to-solid coupling model is meshed with S4R shell elements and C3D20R continuum elements as shown in Figure 3. The continuum meshes used in the static submodeling and shell-to-solid coupling analyses are identical. The continuum meshes extend 10 mm along the pipe length, have a radius of 25 mm in the plane of the plate, and use four layers through the thickness. The continuum meshes accurately model the fillet radius at the joint. Hence, it is possible to calculate the stress concentration in the fillet. The problem could be expanded by adding a ring of welded material to simulate a welded joint (for this case the submodel would have to be meshed with new element layers representing the welded material at the joint). The example could also be expanded by including plastic material behavior in the submodel while using an elastic global model solution.
A reference static solution consisting entirely of C3D20R continuum elements is also included (see Figure 4). The mesh of the reference solution in the vicinity of the joint is very similar to that used in the submodeling and shell-to-solid coupling analyses.
The geometry and material properties of the Abaqus/Explicit shell-to-solid coupling model are identical to the Abaqus/Standard models. The Abaqus/Explicit shell model is meshed with S4R elements, and the continuum model is meshed with C3D10M elements.