Thread Content
This post was last edited by Freestyle-sky on 2018-5-2 at 11:15. Original work is respected; this article comes from the WeChat official account “ANSYS Analysis and Design Professionals”. Example of finite element analysis for flexible thin tube sheets 【1. Determining the initial calculated thickness of the tube sheet】 Taking a composite reactor with flexible thin tube sheets as an example, as shown in the figure below. Since the heat exchange tubes are filled with catalyst and weigh 26.2 tons, ring forgings with good load-bearing capacity were used to connect the lower tube sheet, lower tube box, and shell. The reactor has 6,041 heat exchange tubes, with a specification of Φ38×2; these tubes are arranged at an angle of 60° and are spaced 48 mm apart. The design parameters, materials, and thermophysical property values are shown in the table below: 1. Schematic diagram of the flexible thin tube sheet composite reactor structure. Basic design parameters; the thicknesses of the materials at different temperatures, determined using the flexible thin tube sheet calculation method, are as follows: the thickness calculated according to GB/T150 standards is 7.62 mm ； Calculated according to the SH/T3158 method, the thickness is 6.24 mm ； The thickness of 6.45 mm is calculated according to the West German AD specification method ； According to the GB/T151 calculation method, it is 6.14 mm. However, given the large diameter of this equipment, significant deformation occurs during the welding of the tube sheet to the heat exchange tubes, which imposes high requirements on the manufacturing processes of the factory. Moreover, since the heat exchange tubes are filled with catalyst, the tube sheet must bear not only the weight of the heat exchange tubes but also that of the catalyst, which has a considerable impact on the deformation of the tube sheet. After numerous calculations using finite element software, a thickness of 24 mm was ultimately chosen for this flexible thin tube sheet. 【2. Establishment of the finite element model】 I. Model simplification: (1) Considering the large size of the entire model and the large number of heat exchange tubes, a 1/12 symmetric finite element model was established ； (2) To simulate the effect of catalyst weight on the tube sheet, as well as the coordination issues related to the deformation of the upper and lower tube sheets, the tube bundle, and the shell, the entire length of the heat exchange tubes was considered ； (3) It is assumed that the tube sheet and heat exchange tubes have a fully penetrated structure, with them being closely bonded together, and contact issues are not considered. II. Element selection: (1) During thermal analysis, the heat exchange tubes are meshed using Solid70 elements, while the remaining structures are meshed using Solid90 elements ； (2) During structural stress analysis, the thermal elements are converted into Solid185 and Solid186 elements respectively. III. Mesh division: (1) The entire model is divided into several individual parts at the locations where the structures are discontinuous, and a SWEEP meshing method is used to create a full hexahedral mesh ； (2) SIZING is used to equally divide the edges in the areas of particular stress concern, thereby refining the local mesh and improving computational efficiency while maintaining accuracy; the overall model mesh consists of approximately 1.5 million nodes. IV. Application of load: (1) The corresponding design pressures are applied to the tube side and shell side respectively ； (2) Considering the pressure drop across the catalyst bed and the hydrostatic pressure of the liquid column, an equivalent pressure is applied to the upper surface of the upper tube box ； (3) Consider the effect of structural self-weight. V. Application of boundary conditions: (1) Apply symmetric constraints on all faces at 0 degrees and 30 degrees respectively ； (2) Apply a vertical displacement constraint to the lower end surface of the lower tube box cylinder. 【3. Results of thermal-structural coupling analysis】 As can be seen from the graph, the maximum stresses in the upper and lower tube sheets are 174.1 MPa and 122.4 MPa respectively, both occurring at the edge areas of the tube sheet piping zones; the stress levels decrease in a fluctuating manner as one moves from the edges toward the center of these piping zones. The bundle stress consists of two parts; one part is the primary stress caused by the pressure on the bundle support plate ； The other part consists of the secondary stresses generated by the bending moments and shear forces at the tube sheet edges due to the deformation of the tubes and the shell; these stresses decrease in a fluctuating manner as one moves from the edges toward the center of the tube arrangement. At a distance sufficient from the edge, the value of secondary stress essentially decreases to zero; therefore, in most of the tube routing area of the tube sheet, there is only local bending, with no overall bending caused by the bending moments and shear forces at the edge of the tube sheet. In other words, most tube bundles experience only primary stress. The maximum vertical displacements of the upper and lower tube sheets were 16.1 mm and 5.1 mm respectively, with a small difference in displacement between the center and the edges of the tube sheets, neither exceeding 8 mm. 【4. Structural Stress Strength Assessment】 To provide a more intuitive view of the stress distribution in various areas of the composite reactor, 12 paths were defined within the structure. As can be seen from the data in the table, the stress level in the tube sheet is lower in the tube arrangement area, while it is higher in the edge areas ； The stress values in the upper and lower tube sheet transition sections, as well as in the upper tube bank transition section, are relatively high, and they are mainly caused by bending stress. The stresses of the structure under the remaining operating conditions have all passed the strength assessment; due to space constraints, they are not listed one by one here. 【5. Evaluation of heat exchange tube stability and pulling force】 The stability and pulling force of heat exchange tubes are evaluated in accordance with GB/T151-2014. Based on the finite element calculation results, the maximum axial tensile and compressive forces on the heat exchange tubes under each operating condition can be determined. According to Section 7.3 of GB/T151-2014, the allowable axial compressive stress for heat exchange tubes is as follows: when calculating the pulling force on the welds that connect the heat exchange tubes to the tube sheet, the larger value between the maximum tensile force and the absolute value of the maximum compressive force is taken. The allowable pulling stress is determined using Table 7-12 of standard GB/T151-2014; it corresponds to half of the smaller of the allowable stresses for the tube sheet and the heat exchange tubes at the design temperature, and this value is 56.75 MPa. Table 5 presents the evaluation results for the stability and pulling force of the heat exchange tubes under conditions 1 to 6. The calculation results show that the axial compressive stress in the heat exchange tubes meets the stability criteria, and the welds between the heat exchange tubes and the tube sheet satisfy the allowable tensile shear stress strength requirements.