5. Finite Element Analysis of Bellows

Transcription

1 5. Finite Element Analysis of Bellows 5.1 Introduction: Traditional design process and stress analysis techniques are very specific for each individual case based on fundamental principles. It can only be satisfactorily applied to a range of conventional component shapes and specific loading conditions using sound theories. Also this design process needs continuous improvement till the product becomes matured and proven successful by customers. After that the product becomes standardized. This methodology is followed by majority industries for their products. But in case of customized products, every individual product has unique design features. Specific geometric parameters are altered in order to achieve desirable function from the product. Hence, traditional design technique is not much useful because of very frequent changes in the design calculations. Expansion joints are such customized products, which needs to be treated individually for varieties of applications. Every time design procedure is carried out carefully and minor modifications are also required. During traditional design process many ambiguities remains in the mind of designers because of varieties of application areas of expansion joints. Thus, designers normally use higher safety factors in order to minimize risk. This leads to over design components by specifying either unnecessarily bulky cross sections or high quality materials. Inevitably the cost of the product is adversely affected. Finite Element Analysis (FEA) provides a better solution for design and stress analysis in the virtual environment. Finite Element Analysis (FEA) is a computer-based numerical technique for calculating the strength and behavior of engineering structural components. It can be used to calculate deflection, stress, vibration, buckling behavior and many other phenomena. It can be used to analyze either small or large scale deflection under loading or applied displacement. It can analyze elastic deformation, as well as plastic deformation. Finite element analysis makes it possible to evaluate in detail the complex structures, in a computer, during the 139

2 planning of the structure. The demonstration of adequate strength of the structure and the possibility of improving the design during planning can justify the need of this analysis work. The first issue to understand in FEA is that it is fundamentally an approximation. The underlying mathematical model may be an approximation of physical system. The finite element itself approximates what happens in its interior with the help of interpolating formulas. In the finite element analysis, first step is modeling. Using any special CAD software, model can be generated using the construction and editing features of the software. In finite element method the structure is broken down into many small simple blocks called elements. The material properties and the governing relationships are considered over these elements. The behavior of an individual element can be described with a relatively simple set of equations. Just as the set of elements would be jointed together to build the whole structure, the equations describing the behavior of the individual elements are also joined into an extremely large set of equations that describe the behavior of whole structure. The computer can solve large set of simultaneous equations. From the solutions, the computer extracts the behavior of the individual elements. From this, it can get the stress and deflection of all parts of a structure. The stresses will be compared to permissible values of stress for the materials to be used, to see if the structures are strong enough. Interpretation of the results requires knowing what is an acceptable approximation, development of a complete list of what should be evaluated; appreciation of the need of margin of safety, and comprehension of what remains unknown after an analysis. There are many softwares available for finite element analysis, which can be utilized for the engineering applications. They are ANSYS, Pro/Engineer, CATIA, NASTRAN, Hyper Works, I-DEAS etc. 5.2 Overview of FEA Procedure: 1. Modeling of the component 140

3 A model is required to be generated for the component which is to be analyzed. Designer has to choose proper type of element for the analysis. Actually the kind of component behavior is required to be considered at this stage. The model can be either one dimensional, two dimensional or three dimensional. One dimensional model can be generated by using 2 D spar element; two dimensional models can be generated by key points or directly generating two dimensional shapes like rectangle, circle, etc. Here union, intersection and subtraction of area kind of commands are very useful. In case of three dimensional modeling two dimensional shape can be extruded to third direction, or revolve command is useful. Every designer can have own idea for generating model. Many times component is consist of many small parts, hence all parts are required to be modeled, than assembly function is required. Here type of fit can also be selected as per requirements. Pro/Engineer software is facilitating this kind of features. While earlier ANSYS software does not provide assembly feature. This feature is added in workbench module. All softwares are having their distinct features as well as limitations. User has to make proper choice for applications. 2. Descritization of the continuum: The continuum is the physical body, structure, or solid being analyzed. Descritization may be simply described as the process in which the given body is subdivided into an equivalent system of finite elements. Elements are nothing but a small portion of the continuum which represents the whole continuum that is being analyzed. The finite elements may be triangles, groups of triangles or quadrilaterals for a two dimensional continuum. For three dimensional analysis, the finite elements may be tetrahedral, rectangular prisms or hexahedral. In some cases the extent of the continuum to be modeled may not be clearly defined. Only a significant portion of such a continuum needs to be considered and descritized. Indeed, practical limitations require that on should include only the significant portion of any large continuum in the finite element analysis. 3. Selection of the displacement models 141

4 The assumed displacement functions or models represent only approximately the actual or exact distribution of the displacements. A displacement function is commonly assumed to be a polynomial and practical considerations limit the number of terms that can be retained in the polynomial. The simplest displacement model that is commonly employed is a linear polynomial. Obviously, it is generally not possible to select a displacement function that can represent exactly the actual variation of displacement in the element. Hence, the basic approximation of the finite element method is introduced at this stage. There are interrelated factors which influence the selection of a displacement model. Usually, since a polynomial is chosen, only the degree of the polynomial is open to decision. The particular displacement magnitudes that describe the model must also be selected. These are usually the displacements of the nodal points. 4. Derivation of the finite element stiffness matrix: The stiffness matrix consists of the coefficients of the equilibrium equations derived from the material and geometric properties of an element and obtained by use of the principle of minimum potential energy. The stiffness relates the displacements at the nodal points (the nodal displacement) to the applied forces at the nodal points (the nodal forces). The distributed forces applied to the structure are converted into equivalent concentrated forces at the nodes. The equilibrium relation between the stiffness matrix [k], nodal force vector {Q}, and nodal displacement vector {q} is expresses as a set of simultaneous algebraic equations, [k] {q} = {Q} (5.1) The elements of the stiffness matrix are the influence coefficients. A stiffness of a structure is an influence coefficient that gives the force at one point on a structure associated with a unit displacement of the same or a different point. The stiffness matrix for an element depends upon (1) the displacement model, (2) the geometry of the element, and (3) the local material properties. For an elastic isotropic body, a pair of parameters such as the young s modulus E and the Poisson s ratio define the local material properties. Since material 142

5 properties are assigned to a particular finite element, it is possible to account for non-homogeneity by assigning different material properties to different finite elements in the assemblage. 5. Assembly of the algebraic equations for the overall descritized continuum. This process includes the assembly of the overall or global stiffness matrix for the entire body from the individual element stiffness matrices, and the overall global force or load vector from the element nodal force vectors. The most common assembly technique is known as the direct stiffness method. In general, the basis for an assembly method is that the nodal interconnections require the displacements at a node to be the same for all elements adjacent to that node. The overall equilibrium relations between the total stiffness matrix [K], the total load vector {R}, and the nodal displacement vector for the entire body {r} will again be expresses as a set of simultaneous equations. [K] {r} = {R} (5.2) These equations can not be solved until the geometric boundary conditions are taken into account by appropriate modification of the equations. A geometric boundary condition arises from the fact that displacements may be prescribed at the boundaries or edges of the body or structure. 6. Solutions for the unknown displacements The algebraic equations assembled in above step are solved for the unknown displacements. For liner equilibrium problems, this is a straightforward application of matrix algebra techniques. For non-linear problems, the desired solutions are obtained by a sequence of steps, each step involving the modification of the stiffness matrix and/or load vector. 7. Computation of the element strains and stresses from the nodal displacement In certain cases the magnitudes of the primary unknowns, that is the nodal displacements, will be all that are required for an engineering solution,. More often, other quantities derived from the primary unknowns, such as strains and/or stresses, must be computed. 143

6 The stresses and strains are proportional to the derivatives of the displacements and in the domain of each element meaningful values of the required quantities are calculated. These meaningful values are usually taken as some average value of the stress or strain at the center of the element. 5.3 The basic Element Geometry: When modeling any structural problem, the geometry must be split in to a variety of element. To do this, elements essentially have one of the five basic forms shown in table 5.1. Table 5.1: Basic forms of Elements Dimensionality Type Geometry Point Mass Line Spring, beam, bar, spar, gap, torsion Area 2D continuum, axi-symmetric continuum, plate or flat shell Curved Area Generalized shell Volume 3D continuum 5.4 Typical range of elements: Finite element solutions program has a library of element types it understands. The model must be built using only these supported elements if we want to solve the model in solution. The elements supported for the different analysis types are presented in the table

7 Element Type Degrees of Freedom Mass - Table 5.2: Types of Elements Representations 2D bar u, v 2D beam v, Oz 2D continuum plane stress plane strain axisymmetric 2D interface u,v u,v Axisymmetric shell u,v, Oz 3D bar u, v, w 3D beam u, v, w, Ox, Oy, Oz 3D solid u, v, w 3D Shell u, v, w, Ox, Oy, Oz 3D interface u, v, w 145

8 5.5 The Rules for Compatibility: If elements are compatible internally and across their boundaries then, as the mesh is refined, the solution will coverage to the exact solution of the finite element method. Element must have the same order, although one can mix three sided and four sided elements. There must be connection between the nodes of adjacent elements if the element is 1 D, between the edges of adjacent elements if the element is 2 D and between faces of adjacent elements if the element is 3 D. 5.6 Structure Material Property: To carry out a successful stress analysis for the purpose of design, analyst must provide the material properties, in particular the elastic constants (Young s modulus and Poisson s ratio) and strengths. Other properties such as thermal conductivity, wear resistance and corrosion allowance may be relevant to the product function. A body is homogenous if it has identical properties at all points, and It is considered as isotropic when its properties do not vary with direction or orientation. The property, which varies with orientation, is said to be an isotropic property. Metal becomes anisotropic when they are deformed severely in a particular direction, as happens in rolling and forging. 5.7 Meshing: The arrangement of the elements through the continuum is known as the form or topology of the mesh. The elements can be arranged in any manner, provided that the faces of the elements are positioned correctly. This means that to ensure compatibility of the mesh, the edges of two-dimensional and the faces of three dimensional elements, which are touching, must be in contact, with edge exactly matching edge or face exactly matching face and with node matching node.there are two ways in which the mesh structure can be arranged. The first is the regular form (topology) or irregular form. 146

9 5.7.1 Free and Mapped Meshing: Nodes and elements are generated by one of the two methods, mapped or free mesh. Mapped meshing requires the same number of elements on opposite sides of the mesh area and requires that mesh areas are bounded by three or four edges. If one defines a mapped mesh area with more than four edges, one must define which vertices are the topological corners of the mesh. Mapped mesh boundaries with three corners will generate triangular elements Mesh Refinement: Once the mesh has been generated, it is possible to modify it in such a way that the better solution can be produced. On many occasions the solution will be good over most of the model but will need refinement / enrichment in one or two regions. Mesh modification technique can be applied after a solution has been produced on an initial mesh. There are three ways to refine mesh, H refinement, P refinement and HP refinement Mesh Enrichment: The original mesh has regular spacing but enrichment is required near to stress concentration area. Here more number of nodes and elements are generated in the mesh enrichment Quality Criteria of meshing: New generation Computer Aided Engineering (CAE) softwares have very useful meshing features. Modern software consists of wide range of meshing characteristics. The main objective for the quality mesh are control on size of elements, coarse or fine mesh, addition and removal of node points depending on surface, and editing features of elements. They define all these features through measure of certain quality criteria of meshing. They are described bellow Aspect ratio: Quadrilateral area will have four side characteristics. Other shape may be divided into triangles. An aspect ratio is defined as the ratio of maximum to minimum characteristic of dimensions. Equilateral triangular configurations are best elements. But it is very difficult to achieve all elements of similar size. Therefore practically at least 70% elements should have similar size. 147

10 Maximum angle: The corner angles of an element will have variable values in terms of degree. The maximum angle should be up to Minimum angle: The corner angles of an element will have variable values in terms of degree. The minimum angle should be at least Biasing The biasing sub-panel allows the user to control the distribution of nodes during the nodes seeding by selecting biasing in the form of linear, exponential or bell curve distributions. Figure 5.1 shows basing node arrangement. Figure 5.1 : Biasing of nodes along length Skew: The skew angle is the difference between right angle and angle of a parallelogram. For homogeneous element arrangement the minimum and maximum skew angles are observed. The minimum difference is always preferable in skew angle Morphing: This is a mesh morphing tool that allows user to alter finite element models while keeping mesh distortions to a minimum. Morphing tool can be also useful to: Change the profile and the dimensions of mesh Map an existing mesh onto a new geometry, and Create shape variables that can be used for optimization Masking: The masking tools allow the user to show and hide select entities that might interfere with desired visualization. 148

11 5.8 Restraints: Restraints are used to restrain the model to ground. Restraints also have six values at nodes; three translations and three rotations. Each entry can either have a value for the fixed displacement or is left free to move. 5.9 Constraints: Constraints are used to constrain nodes to other nodes, not to ground. They can be used to impose special cases of symmetry boundary conditions, or special relationships between nodes Structural Loads: Structural loads can be nodal forces or pressures on the face or edge of an element. A nodal force has six values for three forces and the three moments Boundary Conditions: Any analysis case consists of model subjected to constraints, restraints, structural loads and heat transfer or other similar scalar field loads. The boundary conditions are applied to build analysis cases containing loads and restraints of the model. In finite element analysis, the model is considered to be in equilibrium. So the loads and the moments should be such that the equilibrium condition satisfied. ΣF = 0 & ΣM = 0 (5.3) If the end condition of the model is not applied to the model then the reaction at that point or edge or surface should be applied to make it in equilibrium. Boundary conditions can be applied to the part geometry before meshing or the resulting nodes and elements after meshing. Applying boundary conditions to the part geometry will mean that if the part is changed and the model is updated, the boundary conditions will also be updated. There are two special cases of boundary conditions; symmetry and antisymmetry, which can be utilized for as per requirement Computer Aided Engineering softwares: Various softwares are available for the finite element analysis. All are having different area of specialization. Some softwares like Pro/Engineer, I-DEAS, Mechanical Desk Top etc. are having very wide range of modeling features. 149

12 Hyper-Mesh software is good at meshing or descrtization features. CosMos, LS- Dyna, ANSYS etc. are good at engineering analysis. Effluent is specialized for Computational Fluid Dynamics (CFD) Linear Analysis and Non-linear Analysis: When one could not achieve accuracy in the solution from linear finite element analysis, non-linear methodology should be utilized. A nonlinear solution is a series of successive linear steps (iterations) along a path that is not straight. But nonlinear solutions require more data and it takes more time to setup and solve. Most of the world is nonlinear. In many cases, simply understanding the effects of the nonlinearity can enable a design engineer to make sound design decisions on linear results. All problems could be run as nonlinear analyses, but it should be used when only it is necessary Types of nonlinear behavior: Following are the types of non-linear solutions. Yielding/plasticity (beyond Hooke's law: s = Ee) Changing contact or interference Large displacement, large rotation, large strain, stress stiffening Manufacturing processes (mold filling, forging, rolling, stamping, welding) 150

13 5.14 Stress Analysis using FEA: The bellows are designed by customized approach for individual application. The prototype testing is highly time consuming and costly task. Also, the measurement of stresses is very difficult part during the testing bellows. Hence, computer based Finite Element Analysis will be very much useful for the designers to estimate the stresses for newer geometry bellows. This exercise is carried out with the objective that the stresses can be estimated of bellows with FEA methodology. This technique will be beneficial to designers and manufacturers for faster design and analysis. The primary function of expansion joint is to absorb axial (longitudinal), perpendicular (lateral) and angular motions in the long piping and ducting. The bellows are most critical part of expansion joint assembly, which takes of all these movements of piping. Figure 5.2 shows axial movement of metallic bellows. Figure 5.2: Axial Motion of bellow The motions or movements are developed because of differential variation in pressure and temperature inside the long piping. Many times shocks are also developed because of sudden stop and start of fluid flow in the piping. The pressure fluctuations and temperature variations creates unpredictable stresses in the piping. Since the bellows are formed from very thin sheet metals, the movement creates deformation in the elastic as well as plastic region. Hence, It is very difficult to estimate the stresses developed in the expansion joint assembly. The induced membrane stresses in the bellow material must be less than the allowable stress of the materials at the design temperatures. The bellow should be flexible in order to get flexibility and tough to resist pressure fluctuations. This conflicting need for thickness for pressure capacity and thinness for flexibility is the unique design problem faced by the expansion joint designers. 151

14 Bellow is made from SS 304 stainless steel sheets. Other properties are mentioned in material properties Geometry of bellows: Figure 5.3: Geometry of a bellow Figure 5.3 shows a bellow with two convolution and single ply material with reference to following geometrical nomenclature. Db = Inside diameter of the pipe / bellow = 30 cm N = Number of convolution = 2 w = Height of convolution = 3.5 cm q = Pitch of convolution = 4.0 cm Lt = Lc = Tangent length and Collar length = 2.5 cm Thickness of materials = 0.05 cm Number of ply of material = 1 1 ELEMENTS AUG :39:51 Z X Y Figure 5.4: Bellow model 152

15 Stresses in metallic bellows: The expansion joints are loaded with internal pressure due to flowing fluid at inner surfaces. In order to get higher flexibility, bellow is made from thin sheet metal. Since the thickness of the material is very less compare to other two dimensions, membrane stress are produced. The stresses are developed in the radial / circumferential direction as cylindrical shape of bellow. The outer cylindrical surface of bellow, undergo maximum stress value, called hoop stress or circumferential stress. The approximate value of this stress can evaluate by following equation number. Circumferential stress = P D 2t (5.4) The stress produced in the longitudinal direction, along the flow of liquid is longitudinal stress or meredional stress. In case of hollow pipes, the longitudinal stress is approximately half the circumferential stress. Longitudinal membrane stress = P w 2ntp (5.5) Longitudinal bending stress = P 2n w tp 2 Cp (5.6) These relationships are based on shape of convolution; they may not give true stress value for all types of bellows. The bellows consists of some number of convolutions, and hence a stress due to bending is produced, which is very high compare to its membrane stress due to fluid pressure. The total longitudinal stress will be combined effect of stress due to membrane and bending. Estimating the stresses produced is depending upon number of parameters. They are internal pressure fluctuations, inside temperature and its variation, material properties, geometrical parameters, convolution shapes, material thickness, number of plies, heat treatment of the material etc. Considering the complexity of the case, accurate prediction of stress is difficult. Many researchers have contributed to develop mathematical models, but the results are varied because of change in the geometry of the convolutions. Hence there is no general purpose solution available to this. 153

16 The EJMA has developed the codes for evaluation of stresses. This includes finer details of the shape of bellow and estimates precise stresses. Actual experimentation is possible but it is very difficult to measure the various stresses developed. Therefore computerized technique is more convenient for the stress analysis 2. Even one researcher has suggested that consideration of strain concentration can be also a useful approach for the greater accuracy in design of bellows. In the present study ideal geometry U - shape of convolutions are selected. Finite Element Analysis carried out using ANSYS software. Assumptions for the analysis: 1. The material used is homogeneous and isotropic. 2. The material thickness is uniform throughout its cross section. 3. The inside temperature is room temperature and it is constant. 4. The deformation taking place is within elastic limit. Material obeys Hook s law of elasticity. 5. All convolutions are equal in size at pitch distance. Element selection: The important task at the beginning of Finite Element Analysis is selection of type of element. Bellow material have very less thickness, hence shell element should be selected. There are various shell elements which can be used for the analysis. They are Shell 28, Shell 41, Shell 43, Shell 63, Shell 93, Shell 143, Shell 150, and Shell 181. Here shell 181 element is chosen for the analysis which is having following features. SHELL181 is suitable for analyzing thin to moderately-thick shell structures. It is a 4-node element with six degrees of freedom at each node: translations in the x, y, and z directions, and rotations about the x, y, and z-axes. In case of membrane option used, the element has only translational degrees of freedom. The degenerate triangular option should only be used as filler elements in mesh generation. 154

17 SHELL181 is well-suited for linear, large rotation, and/or large strain nonlinear applications. Change in shell thickness is accounted for in nonlinear analyses. In the element domain, both full and reduced integration schemes are supported. SHELL181 accounts for follower (load stiffness) effects of distributed pressures. SHELL181 may be used for layered applications for modeling laminated composite shells or sandwich construction. Material properties: The bellow material is SS 304 sheets. It possess following properties. Modulus of elasticity, E = Poisson s ratio = 0.3 Yield stress of the material, Sy = Allowable stresses of the material, Sab = Coefficient of Thermal Expansion, α = 17.3 x 10-6 m/m K. Reference temperature, T = 273 K. Uniform temperature = 300 K. Constraints: As the expansion joints are fixed through the collar at both ends. The displacement constraint is made fixed at tangent length on both sides. The inside fluid pressure will be acting on inner wall of convolution as well as tangent area. Collars are not included in the model; hence its effect should be neglected for stress evaluation. It is also assumed that the fluid pressure is to be born by convolutions only. Tangent length of bellow = Ux = Uy = 0 Loading conditions: The material properties are given for the analysis as following. The element shell 181 is suitable for analyzing thin to moderately-thick shell structures. It is a 4- node element with six degrees of freedom at each node: translations in the x, y, and z directions, and rotations about the x, y, and z-axes. Change in shell 155

18 thickness is accounted for in nonlinear analyses. It is may be used for layered applications for modeling laminated composite shells or sandwich construction. In actual practice the bellows are pressurized by high pressure fluid flow. In the present study, this is simplified by applying uniform pressure at inside surfaces of bellow. The pressures (gauge) at inside surface are taken as 2.5, 5, 7.5 and FEA Results: Table 5.3: FEA Results from ANSYS Gauge Pressure Deflection, cm Circumferential stress Longitudinal stress FEA result images are shown in figure 5.5 and 5.6. It shows that the maximum stresses are developed near to root area of the convolutions. This is because of stress concentration effect. The maximum stresses are surrounding the root diameter because of its symmetrical shape Analytical Results: Table 5.4: Analytical Results Gauge Pressure Circumferential stress Longitudinal stress Table 5.4 shows analytical results of stresses of bellows calculated using EJMA codes. Results are compared at gauge pressure of 10. Analytical results are calculated using equations 5.1, 5.2 and

19 1 ELEMENT SOLUTION STEP=1 SUB =1 TIME=1 SX (NOAVG) RSYS=0 DMX = SMN =-1016 SMX = SEP :18:23 Y Z X MN MX Figure 5.5 : Results from FEA Figure 5.6 : Stress distribution 157

20 Circumferential stress = P D 2t = 10 x 30 2 x 0.05 = Longitudinal membrane stress = P w 2ntp = 10 x3.5 2 x1x = 372. P w Longitudinal bending stress = Cp = 2n tp 2 x x0.425= Total longitudinal stress = = Longitudinal membrane & bending stress Sab x Factor for formed bellow x 3 = 38214; stresses are within safe limit Graphs: Displacement, cm Pressure, Displacement Figure 5.7: Nodal Displacement 158

21 Stresses, Pressure, Circumferential stress Longitudinal stress Figure 5.8: Stresses developed in bellows vs pressure (FEA) Circumferential stress, Pressure, FEA Analytical Figure 5.9 : Comparison of Circumferential stress 159

22 Longitudinal stress, Pressure, FEA Analytical Figure 5.10 : Comparison of Stress intensity (longitudinal) Stress distribution in the bellow: The stresses developed due to loading can be visualized as per their location. Some node locations are selected as showing in figure The values of resultant stresses are shown in appendix C. Figure 5.11 : Selected nodal point locations for stress analysis The results of stresses are plotted as per node location are shown in figure 5.12 and figure They show distribution of longitudinal stresses and distribution of circumferential stresses at selected nodes. 160

23 Maximum stress intensity (Longitudinal) Maximum stress intensity, Location Number Figure 5.12: Longitudinal stress distribution Figure 5.10 shows that the maximum longitudinal tensile stresses are developed at location number 5, 6, 11, 12, & 13. The longitudinal stress at tangent length is tends to zero. The longitudinal stress is maximum at convolution faces and root area, while it is minimum at crest of convolution. Circumferential stress distribution 3000 Circumferential stress, Location number Figure 5.13: Circumferential stress distribution Figure 5.13 shows that the circumferential compressive stresses are developed at location number 3, 4, 7, and 8. The maximum tensile circumferential stresses are developed at 12. This is root area of bellow, which undergoes very high 161

24 compressive stress. The bellow convolution will be deflected due to loading. The displacement of each node is listed in table 5.5. Table 5.5: Displacement at various nodes Location No. Node No. δx δy The displacement curve as per absolute co-ordinates is plotted in figure The deformation curve shows that the deflection is uniform and maximum is near to convolution flank, which is developing longitudinal stress. Figure 5.14 : Displacement curve of convolution surface 162

25 Observations: 1. Nodal displacement (axially) increases with increase in internal pressure of bellow. (Figure 5.7) Circumferential stresses and longitudinal stresses increase with increase in pressure. (Figure 5.8) The stresses developed are well within the permissible limit of the material. 2. Longitudinal stresses are higher than circumferential stresses. This is because of bending effect at convolution faces. As stresses because of bending is always higher than direct stresses causes due to fluid pressure. This is agreeable to the analysis of EJMA. 3. Maximum stresses produced at the root area of bellow. This is due to stress concentration effect. The remedial action can be taken to control the stresses as convolution rings can be used at root area. Infect, U shape convolution geometry produces minimum stress concentration effect compare to any other shape of convolutions. 4. Stresses calculated by FEA are near to analytical values. This validates the results derived from FEA. The variations are up to 13%. 5. Since, experimentation and actual prediction of stresses developed in the metallic bellows are difficult to predict and measurement incase of experimentation hence, this methodology can be very much helpful in practical applications Axi-symmetry Approach of FEA: Many objects have some kind of symmetry like axi-symmetry, repetitive (cyclic) symmetry or reflective (mirror image) symmetry. An axi-symmetry is observed in many engineering components like metallic bellows, flywheel, arms of flywheels, coupling, light bulb etc. Repetitive symmetry can be visualized in evenly spaced cooling fins on a long pipe, teeth of gears along pitch circle diameter etc. The reflective symmetry can be visualized in connecting rod, moulded plastic containers. When an object is symmetric about center line, one can often take advantage of that fact to reduce the size and scope of the model in Finite Element Analysis. 163

26 Symmetric object means similarity in geometry, loads, constraints, and material properties Axi-symmtery Structures: Any structure that displays geometric symmetry about a central axis in case of shell or solid of revolution in any object is an axi-symmetric structure. Examples would include straight pipes, cones, cylindrical vessels, circular plates, domes, flywheels, couplings and so forth. ANSYS software suggests that, models of axi-symmetric 3-D structures may be represented in equivalent 2-D form. One can expect that results from a 2-D axisymmetric analysis will be more accurate than those from an equivalent 3-D analysis [3]. By definition, a fully axi-symmetric model can only be subjected to axi-symmetric loads. In many situations, however, axi-symmetric structures will experience nonaxisymmetric loads. In this case one must use a special type of element, known as an axi-symmetric harmonic element, to create a 2-D model of an axi-symmetric structure with non-axisymmetric loads Requirements for Axi-symmetric Models Special requirements for axi-symmetric models include: 1. The axis of symmetry must coincide with the global Cartesian Y-axis. 2. Negative nodal X-coordinates are not permitted. 3. The global Cartesian Y-direction represents the axial direction, the global Cartesian X-direction represents the radial direction, and the global Cartesian Z-direction corresponds to the circumferential direction. 4. Unless otherwise stated, the model must be defined in the Z = 0.0 plane. The global Cartesian Y-axis is assumed to be the axis of symmetry. Further, the model is developed only in the +X quadrants. Hence, the radial direction is in the +X direction. 5. Model should be assembled using appropriate element types. For axi-symmetric models, use applicable 2-D solids with plane stress, plane stress with thickness or axi-symmetry option. The model can be created using 164

27 3-D axi-symmetric shells also. In addition, various link, contact, combination, and surface elements can be included in a model that also contains axisymmetric solids or shells. The program will not realize that these "other" elements are axi-symmetric unless axi-symmetric solids or shells are present Guidelines for Modeling: Small details that are unimportant to the analysis should not be included in the solid model, since they will only make your model more complicated than necessary. However, for some structures, "small" details such as fillets or holes can be locations of maximum stress, and might be quite important, depending on your analysis objectives. One must have an adequate understanding of the structure's expected behavior in order to make competent decisions concerning how much detail to include in the model. In some cases, only a few minor details will disrupt a structure's symmetry. One can sometimes ignore these details, in order to gain the benefits of using a smaller symmetric model. Designer must weigh the gain in model simplification against the cost in reduced accuracy when deciding whether or not to deliberately ignore unsymmetrical features of an otherwise symmetric structure. If the structure contains a hole along the axis of symmetry, one has to provide the proper spacing between the Y-axis and the 2-D axisymmetric model. Figure 5.15 shows a metallic bellow, which is formed type and made from thin sheets. Its geometry is symmetric about the axis. The metallic bellows are used in piping as a flexible element to take the axial, lateral and angular variations occurring in the piping. The variations are because of fluctuation in pressure and temperature. Figure 5.15: Shape of a metallic bellow 165

28 To analyze this component, axi-symmetry option can be utilized as shown in other sketch. This analysis gives nearby results of the stresses. Here Y axis is axis of symmetry and X axis is the radial direction. Actual Metallic Bellow Figure 5.16: FEA model Metallic Bellow Axi-symmetry model Notations and Dimensions: Number of convolutions = 3 Inside diameter of Bellow = 30 cm Pitch of the bellow = 4 cm Height of convolutions = 3.5 cm Tangent length = 2.5 cm Material properties: Modulus of elasticity = Poisson s ratio = 0.3 Boundary conditions: Tangent lengths of both sides are locked with zero degree of freedom. Loading conditions: Surface pressure selected at inner wall = Results from ANSYS: 166

29 1 ELEMENT SOLUTION STEP=1 SUB =1 TIME=1 SX (NOAVG) RSYS=0 DMX = SMN = SMX = DEC :29:05 Y X Z MN MX Figure 5.17 : Circumferential stress of a bellow using 3 D shell element 1 ELEMENT SOLUTION STEP=1 SUB =1 TIME=1 SX (NOAVG) RSYS=0 DMX = SMN = SMX = DEC :31:44 MN MX Figure 5.18: Axi-symmetry analysis of a bellow 167

30 FEA Results: Table 5.6: FEA Results Type of Analysis 2 D with axi-symmetry option (solid element) 3 D model Analysis (shell element) Circumferential stress Longitudinal stress Stresses, Circumferential stress Axi-symmetric Longitudinal stress 3 D shell Figure 5.19: Graph showing comparison of Axi-symmetric and 3D approaches Observations: 1. The use of symmetry allows us to consider a reduced problem instead of actual full size problem. 2. Modeling time is greatly reduced as geometry is simplified. The modeling of axi-symmetry is in 2D plane. 3. For the axi-symmetry geometry model, number of nodes, number of elements and number of equations are reduced compare to actual 3D analysis. 4. For the analytical solution, the order of the total stiffness matrix and total set of stiffness equations are reduced considerably. 5. By taking advantage of symmetric geometry of the components, finite element analysis becomes simple and fast. 6. 2D axi-symmetry analysis may be proven more accurate than an equivalent 3D analysis. 168

31 5.16 Practical considerations in FEA: This exercise is carried out with an objective of considering various practical aspects while performing Finite Element Analysis. A metallic bellow is considered as a case study for the finite element analysis to study above stated objective. For finite element analysis actual and full size component should not be considered for the analysis, but various practical aspects should be taken in to account. There are many practical aspects for FEA. They are planning of the analysis, choosing type of model, use of symmetry, selecting critical area for maximum stresses, meshing quality parameters, aspect ratio of elements, etc. A case study of bellow is considered for Finite Element Analysis for validation of practical considerations. The results are obtained using ANSYS software Practical Considerations in FEA: 1. Planning of the Analysis: Before beginning the model some important decisions must be made by user. The accuracy of results will depend on these decisions; hence they should be taken very carefully. [B1] a) Objectives of analysis: b) Whether the full model or only portion of a physical system is sufficient. c) Details to be included in the model. d) Selection of elements e) Meshing density 2. Choosing type of Model: The finite element model may be categorized as being 2-D or 3-D, and as being composed of point elements, line elements, area elements, or solid elements. Of course, these can be used as combined different kinds of elements as required. 3. Use of Symmetry: The appropriate use of symmetry will often expedite the modeling of a problem. Three types of symmetry can be considered in the modeling [B3]. They are axi-symmetry, repetitive (cyclic) symmetry or reflective symmetry. Appropriate use 169

32 of symmetry in the modeling allows designer to minimize the problem size instead of the actual problem. An axi-symmetry means object is symmetrical about its axis of revolution. The object shapes may be either cylindrical or conical. The examples falls into this category are rotors, cylinders, couplings, pistons, flywheels, electric bulb, bottles or jar, glass, etc. A repetitive symmetry means, similar pattern is repeating either on a straight line or radial line. The examples in this type of symmetry are fins of an engine or worm gear box, metallic bellow, teeth of a rack, spur gear etc. A reflective symmetry means object is symmetrical about any one or two axis. It appears like mirror image on other side of an axis. The examples in this type of symmetry are rectangle plate with a circular hole, bearing cover, plastic container etc. Figure 5.20 shows FEA model representation of bellows considering repetitive symmetry. Single convolution model Bellow with 3 convolutions (FEA model representation) (Actual Problem) Figure 5.20: Axi-symmetry and Repetitive Symmetry of Bellows Notations and Dimensions: Number of convolutions, N = 3 Inside diameter of Bellow, Db = 30 cm Thickness of material, t = 0.05 cm Pitch of the bellow, q = 4 cm Height of convolutions, w = 3.5 cm Tangent length, Lt = Lc = 2.5 cm Material properties: Modulus of elasticity = Poisson s ratio =

33 Boundary conditions: Tangent lengths of both sides are locked with zero degree of freedom. (Ux = 0, Uy = 0) Loading conditions: Surface pressure selected at inner wall = Modeling options: Using axi-symmetric elements either three convolution model is required as per geometry (figure 5.21). Instead of that, since convolutions are repeating at regular pitch distance, one convolution model may be considered for the analysis (figure 5.22). Results are shown in table 5.7. Figure 5.21: Axi-symmetric full size model Figure 5.22: Axi-symmetric one convolution model 1 ELEMENTS SEP :55:58 Figure 5.23: Meshing in solid element 171

34 FEA Results: Table 5.7: FEA Results Circumferential stresses, Longitudinal Stresses, Pressure 1 convolution 3 D model 1 convolution 3 D model model model ELEMENT SOLUTION STEP=1 SUB =1 TIME=1 SXY (NOAVG) RSYS=0 DMX = SMN = SMX = SEP :01:18 MX MN Figure 5.24: ANSYS Results, Deformed shape Stresses, Circumferential stress Repetitive Symmetry Longitudinal stress 3 D shell Figure 5.25: Graph showing comparison of full model and single convolution model 172

35 Observations: 1. In FEA analysis of bellow convolution pattern is repeating periodically at equal distance (pitch). Hence, repetitive geometry concept may be considered and one convolution sufficient for the stress analysis. 2. Bellow consist of symmetrical geometry, axi-symmetric element may be used instead of 3 D shell (full size) model. 3. Axi-symmetry and repetitive geometry features can be used in combination and finite element can be made simpler. 4. Here single convolutions results are compared to three dimensional full size bellow. So, one convolution is sufficient for FEA. The variations in results are within 20%. 5. Simple and smaller size of model provides higher accuracy in the results. 6. Practical aspects should be considered in modeling phase of finite element analysis. Complicated component model can be simplified by use of symmetry, elimination of least affected features etc. This will save modeling and analysis time, as well as an accuracy of results will increases. 173

36 5.17 Comparison of Convolutions Shapes: The bellow consists of optional convolution shapes like U, V, S, toroidal etc. as we desire. Selection of each convolution shape will be based on designers choice, its maximum pressure value and manufacturing facilities available. Each convolution shape will have different effect on the performance of bellow. This exercise is carried out with the objective that, study of various performance characteristics of different shapes of convolution. Generally U shape, V shape, toridal shape are mostly used in application. Hence these three are considered for the study with Finite Element Analysis methodology. Figure 5.26 shows the comparative geometry of these convolutions. Figure 5.28: Shape and Dimensions of Convolutions Notations and Dimensions: Number of convolutions, N = 1 Inside diameter of Bellow, Db = 300 mm = 30 cm Thickness of material, t = 0.05 cm Height of convolutions, w = 45 mm = 4.5 cm Tangent length, Lt = Lc = 25 mm = 2.5 cm Material properties: Modulus of elasticity = Poisson s ratio = 0.3 Boundary conditions: 174

37 Tangent lengths of both sides are locked with zero degree of freedom. (Ux = 0, Uy = 0) Loading conditions: Surface pressure selected at inner wall = FEA Results: U shape V shape Toroidal shape Figure 5.29 : Meshed model of shapes of convolutions Table 5.8: FEA Results of U shape Convolutions Pressure Circumferential stress Axial stress Max. Stress intensity Table 5.9: FEA Results of V shape convolutions Pressure Circumferential stress Axial stress Max. Stress intensity Table 5.10: FEA Results of Toroidal shape convolutions Pressure Circumferential stress Axial stress Max. Stress intensity

38 Graphs: Circumferential stress, U shape V shape Toroidal shape Figure 5.30: Graph showing circumferential stress Longitudinal stress, U shape V shape Toroidal shape Figure 5.31: Graph showing Longitudinal Stress 176

39 Maximum stress intensity, U shape V shape Toroidal shape Graph 5.32: Graph showing maximum stress intensity Observations: 1. The geometry of the convolution should have uniform shape, any sharp change in geometry will create stress concentration effect and which will leads to higher stress development. 2. In case of U shaped convolutions, circumferential stresses are at maximum, while longitudinal stresses are at minimum level. This is because of straight (perpendicular) convolution faces. 3. U shape convolution permits maximum axial displacement (movement) because of root and crest flexibility. It is because of the vertical edges of the convolutions, which permits higher deflection. 4. For toroidal shape convolutions, circumferential stresses are at minimum level, while longitudinal stresses are at maximum level. This is due to its spherical shape, and toroidal convolution can withstand higher amount of stresses compared to other types of convolutions. 5. Toroidal shape do not permit higher axial deflection because of its spherical shape. 6. V shaped convolution performs the stress level between U shape and toroidal shape convolutions. 177

40 5.18 Structural and Thermal Analysis: The design of bellows is very complex as it involves structural and thermal aspects. Structural design point of view, the bellows should be flexible enough to take up movements or deformations causes by pressure fluctuations. The bellows are manufactured using minimum metal thickness in order to get higher deflection. Here many times the bellows are deformed beyond elastic range of material, hence prediction of stresses are very much critical. As the temperature of the piping rises, the modulus of elasticity of the material is decreases; hence resulting in the development of the higher stresses. The combined structural and thermal aspect makes the design of bellows very much critical. The determination of an acceptable design is further complicated by the numerous geometrical parameters involved such as diameter, material thickness, and shape of convolutions, number of convolutions, pitch, height of convolution, number of plies, etc Problem definition: Notations Db = Inside diameter of the bellow = 30 cm N = Number of convolution = 2 w = Height of convolution = 3.5 cm q = Pitch of convolution = 4.0 cm Lt = Lc = Tangent length = 2.5 cm Thickness of materials = 0.05 cm Number of ply of material = 1 Figure 5.33 Geometric Dimensions of a bellow Bellows are made from sheet metal long tube (seam welded in longitudinal direction). Then the convolutions are formed by any metal forming process using dies. Generally U shape of convolutions is preferred. Figure 5.31 shows a bellow with two convolution and single ply material. It shows the basic geometry of a bellow. 178

41 Loading Conditions: In actual practice the inside surface will be pressurized by fluid. Here we can simplify the experiment by applying uniform pressure at inside surfaces of bellow. Pressure at inside surface is taken as Boundary conditions: As the expansion joints are fixed through the collar at both ends. The displacement constraint is made fixed at both sides. The inside pressure will be acting on cylindrical surface as well as convolution area. Tangent lengths at both ends of bellows are covered by collars. Collars are made from comparatively thick material, considering that the stresses are to be bared by convolutions only. The tangent lengths at both ends are considered as zero degree of freedom as these ends are welded to flanges and subsequently to long pipes. Reference temperature is given at 273 K. Uniform temperature is at K, K, K, K, and K are applied at for the stress analysis Results: Reference temperature: 273 K Pressure Temperature 0 K Table 5.11: FEA Results Circumferential stress N /cm 2 Axial stress Max. stress intensity N /cm

42 1 ELEMENT SOLUTION STEP=1 SUB =1 TIME=1 SX (NOAVG) RSYS=0 DMX = SMN =-1016 SMX = MN MX AUG :12:21 Z Y X Figure 5.34: Longitudinal Stresses at uniform temperature K Analytical Approach: Strength of materials decreases with increase in temperature in case of steel. Its modulus of elasticity is reduced because of thermal vibrations of the atoms in the material, and hence to an increase in the average separation distance of adjacent atoms. To consider this parameter, thermal expansion occurs based on its coefficient of thermal expansion. The linear coefficient of thermal expansion (Greek letter alpha) describes by how much a material will expand for each degree of temperature increase. The thermal expansion coefficient for a pipe is also a thermodynamic property of that material. δ = (ΔT) L Where, δ is the elongation of pipe, is the thermal expansion coefficient, ΔT is the change in temperature, and L is the initial length of the pipe. The flexibility of a bellow is an important parameter for the designers. The actual modulus of elasticity is not applicable for the design procedure, as the flexibility 180

43 increases because of its shell structure. The flexibility parameter is based on shell parameter of a bellow. Many researchers has made attempts to find flexibility parameter t of bellow. E for bellows. It depends on geometric parameters like n, b, h, R and E' Figure 5.35 : U shape geometry of a bellow R t x 0.05 Shell parameter of bellow is λ = 2 = 2 b 1 = 0.83 Shell parameter λ = E, 0.83 = E' E', E = Formulation of stress relationship with reference to thermal expansion of bellow is Elongation of pipe δ = (ΔT) L = 12.6 x 10-3 x ( ) x 13 = 4.43 x 10-3 cm stress Actual Modulus of elasticity, E = strain Stress = E x strain = x 4.43x = Using same procedure all values are computed in following table 5.12 Table 5.12: Analytical Results Pressure Change in Temperature Axial Stresses 0 K = = = = =

44 Graphs: Axial stresses, Temperature, K FEA Analytical Figure : Comparison of FEA and Analytical Results Observations: 1. Longitudinal stresses developed in the bellows increases due to increase in temperature, even though the pressure remains constant. 2. The analysis is based on linear relationship, and non linear mode may give some variations in results. The elongation is based on thermal expansion of bellow material. 3. Longitudinal (along axis) stresses and strains are always higher compared to circumferential stresses because elongation takes place along the length of pipe and bellow and stresses due to bending. 4. FEA results are validated with analytical approach for longitudinal stresses developed in bellow. Finite element analysis using ANSYS gives near to realistic results. 182

45 5.19 Stability Analysis: Structural members, which are considerably long in dimensions compare to their lateral dimensions, starts bending (buckling), when their compressive loading reaches to some critical value. Buckling can be defined as the gross lateral deflection of long columns at center sections. Buckling failure of structures mainly depends upon slenderness ratio. Expansion joints are used in the piping to take deviations occurring because of temperature and pressure variations. These deviations may be axial, lateral and combined. Bellow is a critical element of an expansion joint assembly. Bellows are normally loaded with internal pressure along with elevated temperature depending upon the applications. Design of bellow is very much critical as there are many geometric parameters and many other affecting factors. The stresses developed in the bellows are due to pressure and deflection. Some times bellows becomes unstable because of excessive internal pressure. This kind of failure of bellows is termed as squirm Squirm in Expansion Joints: Expansion Joints Manufacturers Association (EJMA) has established the codes for design of bellows considering buckling. This analytical approach is based on Euler s theory and gives near to realistic estimation of buckling load. This exercise is an attempt to check the bellow for buckling failure using ANSYS finite element method. The squirming phenomenon was first demonstrated by Haringx [2], who showed pressure buckling of bellows was analogous to buckling of Euler strut. He gave following relationship. E I P' 2 2 r l Excessive internal pressure may cause a bellow to become unstable and squirm. Bellows performance is depending on critical pressure. The pressure capacity is decided based on squirm by keeping some factor of safety. Fatigue also depends on squirm pressure. There are two basic types of squirm, column squirm and inplane squirm. 183

46 Figure 5.37 : Column Squirm Figure 5.38 : In-plane squirm Column squirm is defined as a gross lateral shift of the middle section of the bellow. In-plane squirm is defined as deflection occurred in individual convolutions, parallel to the surface of bellow materials. Squirm is associated with length to diameter ratio, called slenderness ratio. According to slenderness ratio, bellows can be categorized in long or short columns. Failure of column depends on the kind of column. Squirm is similar to buckling of column under compressive load. Buckling failure consists of an elastic and in-elastic deformation. Since bellows are made from thin sheet metal, deformation of bellows exists in elastic and plastic region. Hence determination of critical pressure is essential to avoid squirm failure. Buckling analysis is a technique used to determine buckling load or critical load at which a structure becomes unstable or buckle mode shapes - the characteristic shape associated with a structure's buckled response. Eigenvalue buckling analysis predicts the theoretical buckling strength (the bifurcation point) of an ideal linear elastic structure. An eigenvalue buckling analysis of a column will match the classical Euler solution [5]. However, imperfections and nonlinearities prevent most real-world structures from achieving their theoretical elastic buckling strength. Thus, eigenvalue buckling analysis often yields unconservative results. The non linear analysis gives much accurate results. 184