Optimal finite element modelling for modal analysis of liquid storage circular tanks
|
|
- Randolph Bridges
- 6 years ago
- Views:
Transcription
1 Int. J. Structural Engineering, Vol. 5, No. 3, Optimal finite element modelling for modal analysis of liquid storage circular tanks Said A. Elkholy* Civil and Environmental Engineering Department, United Arab Emirates University, P.O. Box 15551, UAE and Fayoum University, P.O. Box 63514, Cairo, Egypt *Corresponding author Alaa A. Elsayed Fayoum Univresity, P.O. Box 63514, Cairo, Egypt Bilal El-Ariss Civil and Environmental Engineering Department, United Arab Emirates University, P.O. Box 15551, UAE Safaa A. Sadek Fayoum University, P.O. Box 63514, Cairo, Egypt Abstract: Model analysis of liquid storage vertical tanks is a complex task due to fluid-structure-soil interaction. Analysis of tanks subjected to earthquake excitations using finite element modelling (FEM) has become a preferred technique. The FEM is validated by comparing its results with experimental and theoretical results in the literature. However, most finite element studies in literature do not provide enough details on the selection of the used. The objective of this study is to provide optimal FEM options of parameters such as element types and number of which best predict the tank dynamic characteristics, natural frequencies and principal mode shapes. Coupled natural frequencies in sloshing modes were obtained for various tank height-to-diameter ratios, various tank wall thicknesses and various liquid depths. The FEM predictions compared well with literature available experimental and numerical results. A set of FEM options of parameters is recommended for elastic and inelastic analysis of such tanks. Copyright 2014 Inderscience Enterprises Ltd.
2 208 S.A. Elkholy et al. Keywords: liquid storage tank; finite ; modal analysis; FE modelling;; sloshing modes. Reference to this paper should be made as follows: Elkholy, S.A., Elsayed, A.A., El-Ariss, B. and Sadek, S.A. (2014) Optimal finite element modelling for modal analysis of liquid storage circular tanks, Int. J. Structural Engineering, Vol. 5, No. 3, pp Biographical notes: Said A. Elkholy is an Associate Professor of Structural Engineering in the Department of Engineering at Fayoum University. He obtained his PhD degree from Tokyo University, Japan and his MSc degree from Cairo University, Egypt. Alaa A. Elsayed is an Associate Professor of Structural Engineering in the Department of Civil Engineering at the Fayoum University. He obtained his PhD degree from the University of Windsor-Canada and his MSc degree from Cairo University, Egypt. Bilal El-Ariss is an Associate Professor of Structural Engineering in the Department of Civil and Environmental Engineering at the United Arab Emirates University. He obtained his PhD degree from Quebec, Canada and his MSc degree from Missouri, USA. Safaa A. Sadek is an Assistant Lecturer in the Civil Engineering Department, Fayoum University, Egypt. She obtained her MSc degree from Fayoum University, Egypt. 1 Introduction Damages to liquid storage tanks in past earthquakes have shown how critical they are to any society and; therefore, have attracted special attention to evaluating the seismic behaviour of such tanks. The most commonly used type of tanks is the vertical thin walled cylindrical tanks. Thin walled cylindrical liquid storage tanks have a simple geometry, but exhibit complex vibration behaviour. This vibration behaviour is a coupled system between the liquid and the tank structure because the tank walls are elastic and deformable. In the coupled system, various vibration modes simultaneously occur during earthquakes because the natural frequencies of most of the modes are in the exciting frequency range of the earthquakes. Seismic behaviour of elastic vertical tanks, whether they are fully or partially filled with liquids, is affected by the tank structural flexibility, fluid properties and soil characteristics. To fulfil the requirement of keeping these tanks functional after a major seismic excitation event, numerous theoretical and experimental studies have been performed to better analyse the seismic behaviour of these tanks. Housner (1963) developed the most commonly used analytical model in which hydrodynamic pressure induced by seismic excitations is separated into impulsive and convective components using lumped mass approximation. This model has been adopted with some modifications in most of the current codes and standards. Yang (1976) used a
3 Optimal FEM for modal analysis of liquid storage circular tanks 209 single degree of freedom model with different modes of vibrations to study the effects of wall flexibility on the pressure distribution in liquid and the corresponding forces in the tank structure. Veletsos and Yang (1977) developed flexible anchored tank linear models and found that the magnitude of the pressure was highly dependent on the wall flexibility. Minowa (1980, 1984) carried out experimental studies investigating the effect of flexibility of tank walls and hydrodynamic pressure acting on the wall of rectangular tanks. Haroun (1984) introduced a detailed analytical method and performed a series of experiments including ambient and forced vibration tests for rectangular tanks. He used the classical potential flow approach to estimate the hydrodynamic pressure assuming rigid tank walls. On the experimental part, three full scale water storage tanks were tested to determine the natural frequencies and mode shapes of vibrations. Also, Haroun and Tayel (1985) used the finite element method for analysing the dynamic response of liquid tanks subjected to vertical seismic ground motions. Veletsos and Tang (1986) analysed liquid storage tanks subjected to vertical ground motion on both rigid and flexible supporting foundations. Haroun and Abou-Izzeddine (1992) conducted a parametric study of numerous factors affecting the seismic soil tank interaction under vertical excitations. Dogangun et al. (1997) implemented a displacement-based fluid finite element model in the general purpose structural analysis computer code SAPIV to analytically study the effects of wall flexibility on the dynamic behaviour of rectangular storage tanks filled with liquid. Excluding the fluid sloshing of the liquid, Chen and Kianoush (2005) estimated the hydrodynamic pressure in two-dimensional flexible rectangular tanks using the sequential method. Kianoush and Chen (2006) analysed the dynamic behaviour of two-dimensional rectangular tanks subjected to vertical seismic excitations. Their model included impulsive and convective masses in their seismic analysis of two-dimensional rectangular tanks. Livaoglu (2008) studied the dynamic behaviour of a fluid rectangular tank-foundation system with a simple seismic analysis procedure using the interaction effects presented by Housner s two mass approximations for the liquid and the soil foundation system. Dutta et al. (2004) studied the dynamic behaviour of reinforced concrete elevated tanks with soil structure interaction (SSI). The investigation, in the initial phase, evaluates primary dynamic characteristics, impulsive lateral period and impulsive torsional-to-lateral period ratio of such systems incorporating the effect of SSI. Curadelli et al. (2010) studied the dynamic behaviour of elevated liquid storage containers because of the interest in their response to seismic loads (e.g., in the petro chemical industry) and in connection with the structural integrity and reliability analysis of diverse shell components (e.g., in nuclear reactors). Ruifu et al. (2011) used the multiple friction pendulum system (MFPS) to analyse the seismic response of an isolated vertical, cylindrical, extra-large liquefied natural gas (LNG) tanks for large displacements induced by earthquakes with long predominant periods. They compared their analysis results to those in the literature and they did not propose finite element modelling (FEM) in their methodology. Moslemi et al. (2011) considered fluid-structure interaction in liquid containing tanks by developing a finite element technique that implements such interaction. Utilising their developed technique, they were able conclude that investigating liquid sloshing effects in tanks of complex geometries such as conical tanks was possible. The they used for the liquid and tank wall were displacement-based fluid and shell, respectively. Amiri and Sabbagh-
4 210 S.A. Elkholy et al. Yazdi (2011, 2012) addressed experimental and numerical investigations of dynamic parameters, natural frequencies and mode shapes of fixed roof ground supported storage tanks. Three tall liquid storage tanks having similar height of m and different radii of 6.095, 8.00 and m were considered using the finite element package ANSYS. The finite element meshes of tank wall and roof were constructed using Shell181 quadrilateral shell and the fluid region was meshed by Fluid80 quadrilateral fluid. They concluded that the constructed models can serve as a baseline in structural dynamics for future analyses. They did not carry out further investigating on other element types that may yield more representative models of the real structures. Sezen et al. (2008) investigated the parameters influencing the dynamic behaviour of above-ground liquid tanks. They carried out simplified and finite element dynamic analyses of the tanks including the effect of liquefied gas-structure interaction using a ground motion recorded at a nearby site. The simplified proposed analysis was based on a three-mass model. In the ANSYS FEM the reinforced concrete columns were modelled using frame. Quadrilateral four-node-shell were used for stainless tank walls and eight-node-solid were used to model the thick reinforced concrete tank. Fluid inside the tank was modelled using eight-node-brick fluid. Jalali and Parvizi (2012) carried out an experimental work to investigate the effects of different parameters on modal properties of liquid-containing structures. Their experimental results were then used to construct analytical models for these structures using the finite element package, ANSYS. Shell element SHELL63 and fluid element FLUID80 from the ANSYS element library were used in their models which were capable of regenerating the experimental dynamic characteristics of the structures with an acceptable accuracy. Maheri and Abdollahi (2013) conducted a numerical study using ABAQUS to investigate the effects of material degradation due to corrosion on the dynamic buckling of three cone roof ground-based, cylindrical tanks with height-to-diameter ratios (H/D) of 0.40, 0.63 and 0.95, subjected to horizontal seismic-base excitations. They used four-sided doubly-curved shell to model the wall and three-sided shell (S3R) are utilised to model the roof. No liquid element was specified or identified in their study to model the liquid-tank interaction. Therefore, different simplified design provisions for tanks have been developed based on the simplified beam model analytical results reported by Veletsos, Haroun and Housner (Veletsos, 1984; Haroun and Housner, 1981) and on experimental research outputs reported in the literature. These simplified design provisions can be found in codes and standards such as American Petroleum Industry (API) Standard 650 Appendix E Seismic design of storage tanks (1980) or in Eurocode 8-Part 4 Tanks, Silos and Pipelines in Appendix B Seismic analysis procedure for anchored cylindrical tanks (1998). The finite element studies listed above did not provide enough details on the selection criteria of the element types used and did not investigate the effects of other element types available in the programme library on the performance of the tanks. The study also recommends the optimal ANSYS shell element type and number of that best predict the tank dynamic characteristics of natural frequencies and principal mode shapes.
5 Optimal FEM for modal analysis of liquid storage circular tanks Description of the finite element model There are two approaches for modelling liquid storage tanks by using mechanical and FE modelling techniques. The mechanical modelling technique has been defined as a simplified model that had been developed by different researchers and recommended by current major earthquake codes. The approaches for modelling tanks included approaches for modelling the fluid structure interaction (FSI) system and approaches for modelling the SSI system. The FE structural analysis programme, ANSYS (2006) was used in this study to produce the FE modelling needed for the tank dynamic analysis. For the FSI analysis, there are different FE approaches to represent fluid motion such as added mass approach, Lagrangian approach, Eulerian approach, Lagrangian-Eulerian in the FE method, smoothed particle hydrodynamic (SPH) methods and analytical methods such as Housner s two mass representations. The main objective of any FE modelling is to create a mathematical representation of the engineering system that reflects its actual geometry and behaviour. Building FE models in ANSYS requires familiarity with the ANSYS operating manual and element library. Each element in ANSYS has specific properties and behaviours to be defined according to the structure in the problem. 2.1 Modelling of the wall tank The 3D FE model of empty tank was established as surfaces using the pre-processor section in ANSYS. The selection of a suitable element for a given application is not a trivial matter and will directly influence the computational time and accuracy of the results. The ANSYS element library has many different types of shell. This study examined the library available shell properties and concluded that six have properties more appropriate for modelling liquid tank walls than other. These shell types are commonly used by several researchers for modelling tanks with different mesh sizes. Therefore, six different FE models were considered and analysed individually in this study to investigate the choice of each of these six and its total number in the mesh on its corresponding FE model performance and output. The best shell element would be the one whose FE model performance and results are the closest to, or have the least difference with, those results in the literature. The six shell considered in this paper are: 1 SHELL43 with stress stiffening, creep and large plastic strain and deflection capabilities, shown in Figure 1. It is a four-node element and is recommended for modelling moderately-to-thick shell structures. Each node has six degrees of freedom in the x, y and z nodal axes. Linear deformation shapes are used in both in-plane motions. For out-of-plane direction, the element uses a mixed interpolation of tensorial components. 2 SHELL63 elastic shell, shown in Figure 2. It is a four-node shell element and is known of its membrane and bending capabilities. Loads applied normal and in-plane are allowed. Each node of this element has six degrees of freedom in the x, y and z nodal axes. SHELL63 is also known of its large deflection and stress stiffening capabilities.
6 212 S.A. Elkholy et al. 3 SHELL93 is an eight-node shell element, shown in Figure 3. It is well suitable for modelling curved shells. Each node has six degrees of freedom in the nodal x, y and z axes. Deformation shapes are quadratic in both in-plane directions. SHELL93 has large plastic strain, stress stiffening and large deflection capabilities. 4 SHELL143 plastic shell, shown in Figure 4. SHELL143 is well suited to model nonlinear, flat or warped, thin to moderately-thick shell structures. It is a four-node element and each node has six degrees of freedom in the x, y and z nodal axes. SHELL143 has small plastic strain, stress stiffening, creep and large deflection capabilities. 5 SHELL181 finite strain shell, shown in Figure 5. It is well suited for modelling thin to moderately-thick shell structures. This element has four nodes and each node has six degrees of freedom at each node and in the x, y and z nodal axes. It is well-suited for linear, large rotation and/or large strain nonlinear applications. Change in shell thickness is accounted for in nonlinear analyses. It can be used instead of SHELL43 for many problems that have convergence difficulty with SHELL43. 6 SHELL281, shown in Figure 6. According to the authors knowledge, this is one of the most recently introduced by ANSYS. Element SHELL281 is an eight-node element with six degrees of freedom at each nodes: three translations and three rotations about the x, y and z nodal axes. The element is suitable for the analysis of thin to moderately-thick shell structures where it is recommended to use quadrilateral shaped. SHELL281 is recommended for modelling linear and nonlinear strain and large rotation applications. SHELL281 may be used for layered applications for modelling laminated composite shells or sandwich construction. Figure 1 SHELL43 elastic shell
7 Optimal FEM for modal analysis of liquid storage circular tanks 213 Figure 2 SHELL63 elastic shell Figure 3 SHELL93 eight-node structural shell Figure 4 SHELL143 plastic shell
8 214 S.A. Elkholy et al. Figure 5 SHELL181 finite strain shell Figure 6 SHELL281 geometry 2.2 Modelling of the fluid As for the fluid, the ANSYS library has different types of fluid that can be used to model the fluid in 2-D and 3-D problems. In this study, the fluid is divided into a number of 3-D fluid (FLUID80 3-D contained fluid) with eight nodes each node having three degrees of freedom. The fluid element FLUID80 is a modification of the 3-D structural solid element (SOLID45). FLUID80 element, shown in Figure 7, is recommended for modelling fluids within vessels with no net flow rate. The fluid element is suitable for computing hydrostatic pressures and fluid/solid interactions. Acceleration effects, such as in sloshing problems, as well as temperature effects, may be included.
9 Optimal FEM for modal analysis of liquid storage circular tanks 215 Figure 7 FLUID80 3-D contained-fluid element 2.3 Modelling of the FSI The fluid-structure interaction can be modelled by one of two ways. The first is called structure surrounded by water (SSW) and the second one is called water surrounded by structure (WSS). The latter is adopted in this research where the tank wall and fluid are used. In the WSS, the fluid domain is modelled inside the structure domain. 2.4 Coupling equations Fluid element at the boundary should not be attached directly to structural (shell ) but should have separate, coincident nodes that are coupled only in the direction normal to the interface. The FSI is accounted for by properly coupling the coincident nodes that lie in the common faces of the two domains (liquid and wall) in the radial direction. This means that the fluid is attached to the shell wall but can slip in the wall tangential directions and therefore only can exert normal pressures to the tank wall. 2.5 Boundary conditions The tanks studied in this research are assumed to have completely fixed-base. Therefore, all the nodes at the base are assumed to be fixed. 2.6 Master degrees of freedom Master degrees of freedom are required in modal analysis. These are degrees of freedom that describe the dynamic behaviour of the structure. The accuracy of the finite element analysis (FEA) depends greatly on the mesh used. A fairly course mesh is first employed and then refined in areas of interest or high stress. The solving time of the model is dependent on the number of which is determined by the mesh density. A low density is appropriate where the stress is uniform over a relatively large area. However, where there is high concentration of stresses over smaller areas a high mesh density is deployed. The model of a circular tank in this research was drawn in ANSYS using volumes, areas and lines and then the mesh is mapped (map meshing allows precise control of the meshing procedure).
10 216 S.A. Elkholy et al. 2.7 Analysis method The reduced method is widely referred to for modal analyses using the ANSYS fluid. This method is used for the eigenvalue and eigenvector extractions to calculate frequencies and modes shapes including the fluid modes. It utilises householderbisection-inverse iteration to evaluate the eigenvalues and eigenvectors. This method uses a small subset of degrees of freedom, referred to as master DOF which makes is suitable for fast calculations that yield an exact stiffness matrix and an approximate mass matrix [M]. The accuracy of the results, therefore, depends on how well [M] is approximated which in turn depends on the number and location of the master degrees of freedom. 3 Modelling and analysis results A verification example of liquid storage tank tested experimentally by Mazúch et al. (1996) and numerically analysed by Zienkiewicz (2005) using the FEA is presented. The tank different mode shapes and frequencies were experimentally obtained and documented by Mazúch et al. (1996). The different analytical frequencies of the same tank were obtained by Zienkiewicz (2005) without using computer software and without providing details on the types and number of used in the analysis. The example was modelled in this study using the computer programme ANSYS and the model frequency values for different mode shapes were compared to the tank experimental measurements and theoretical solutions obtained by Mazúch et al. (1996) and Zienkiewicz (2005) respectively. 3.1 A three-dimensional experimental tank A 3D flexible circular tank tested by Mazúch et al. (1996) was chosen to verify this study model results. The tank, shown in Figure 8, was tested in two different cases: empty tank case and filled with liquid tank case. The same tank was numerically analysed for both cases by Zienkiewicz (2005) using the FEA method. The available experimental and analytical results were used to verify the accuracy of the results produced by the ANSYS models proposed in this study. In addition, a parametric study was performed to evaluate the effect of some variables on the numerical simulations, such as element types and mesh sizes. Figure 8 Tank tested experimentally by Mazúch et al. (1996)
11 Optimal FEM for modal analysis of liquid storage circular tanks 217 The elastic cylindrical tank had a mean radius R = mm, a wall thickness h = 1.5 mm and a length L = 231 mm; the tank material characteristics were Young s modulus E = N/m 2, Poisson ratio υ = 0.3, density ρ s = 7,800 kg/m 3. Water was used as the contained fluid having a density of 1,000 kg/m 3. The tank was welded at the base to a 20 mm thick circular plate which was bolted to a heavy-base block.the tank was filled with water up to the level H. The boundary conditions of the shell were theoretically assumed to be of clamped-free type. Finite element analyses using ANSYS were performed to obtain the modal characteristics of the tank. The fluid region is divided into a number of three-dimensional contained fluid. The tank is modelled with different types of shell as mentioned above. 4 Empty tank case The experimental natural frequencies and mode shapes of the considered liquid storage tank were obtained from the vibration measurements by Mazúch et al. (1996). The analytical natural frequencies and mode shapes were computed as well by Zienkiewicz (2005). In this study, the empty tank was treated as a 3D empty tank and was modelled as surfaces using the pre-processor section in ANSYS. The bottom nodes of the tank shell are fixed in all six degrees of freedom. The model was drawn in ANSYS using volumes, areas and lines and then was map-meshed (map meshing allows precise control of the meshing procedure). In order to find the best numerical model for the experimental test, a total of 22 FE models of the tank were built in ANSYS, 19 models with four-node shell and three models with eight-node shell. To start modelling the tank, it was first decided to examine the effect of the model s element number increase along the tank circumferential perimeter (radial direction) and along its height on the convergence and accuracy of the tank frequency values obtained. First, the number of divisions along the tank height, N H, was chosen to be ten divisions and kept fixed while increasing the number of divisions along the radial direction, N R, from 6 to 30 divisions. Next, N H was increased to twenty divisions and kept fixed while increasing N R from 6 to 30 divisions. SHELL 43 were used in this model convergence test and the model frequency results were compared to the tank frequency measurements by Mazúch et al. (1996). Figure 9 shows the FE model of the empty tank using ANSYS. Figure 9 3D FE model of empty tank (see online version for colours)
12 218 S.A. Elkholy et al. Table 1 FE model natural frequencies for empty clamped-free cylindrical tanks (Hz) with varying N H and N R NH = 10 NH = 20 SHELL 43 ELEMENT NR = 6 NR = 12 NR = 18 NR = 24 NR = 30 NR = 6 NR = 12 NR = 18 NR = 24 NR = 30 Total no. of Total no. of ,692 2,688 3, ,392 2,412 3,648 5,100 Mode m n Experiment , , ,479 1,624 1, , , , , , ,495 1,486 1, ,628 1,677 1, , , , , , , , , ,851 1,924 1, ,821 1, ,815 1, , ,828 1, , ,969 2,060 2, , , , , , ,046 2, , ,151 2,486 2, , , , , , , , ,167.6
13 Optimal FEM for modal analysis of liquid storage circular tanks 219 Figure 10 Effects of element number increase, N H and N R, on the model result accuracy
14 220 S.A. Elkholy et al. The results of this model test are shown in Table 1 and in Figure 10. Figure 10 shows that increasing the numbers of in both directions, the height of the tank and the circumferential perimeter of the tank, minimises the difference in the model results and the experimental measurements which means increasing the results accuracy. However, it can be concluded that increasing the number of in the radial direction of the tank yields a faster increase in the accuracy of the model results than the accuracy increase when increasing the number of in the tank height direction. Number of in the tank-base would be equal to the total number of generated by ANSYS minus N H *4N R. The tank analysis began with ANSYS models of 252 using the different shell listed above separately. To investigate the effects of the element number in the model on the tank calculated dynamic properties, i.e., natural frequencies and principal mode shapes, the number of over the cylindrical shell surface was increased gradually from 252 to 7,168. The different types of shell above were used separately in the different models of the tank with the different element numbers to check the effects of choosing a particular individual shell element option on the validity and accuracy of the results, therefore to propose the optimal model element types and numbers for analysis of such tanks. In this analysis, a large number of different models were investigated (as shown in Table 2) to obtain the dynamic characteristics of the empty tank. The model mode shapes of the empty tank using ANSYS and those of experimental measurement are shown in Figure 11. A comparison shows good agreement of the results obtained from the FE analysis and the experiments. Therefore, the results demonstrate the validity of the model. The mode shapes of the cylindrical shell are identified by the number of axial modes, m and number of circumferential waves, n. Table 2 shows the experimental natural frequency measurements by Mazùch et al. (1996), the frequency analytical values from FEM by Zienkiewicz (2005) and the natural frequencies predicted by the ANSYS FE models in this study using different element types and numbers. The FE model-obtained frequency results were compared with their corresponding experimental measurements by Mazùch et al. while the analytical values by Zienkiewicz were used as a reference. This comparison is shown in Table 1 as error, or difference, percentages. The less the error or difference, the better the model result accuracy is. As it can be seen in Table 2, the obtained FE results display good pattern with the experimental results verifying that the current method of tank FE modelling can further be employed to study the FSI problems of liquid-containing structures. The table also shows that when using finer mesh, or increasing the number of, the frequencies obtained from the FE models tend to come close to the experimental measurements. The results of the final idealisation (7168 ) compared very well with the experimental measurements, except for the mode shape (m = 1 and n = 2) and they were adopted for the in-vacuum dynamic characteristics of the vertical clamped-free cylindrical shell. The mode shapes of the cylindrical shell are identified by the number of axial modes, m and the number of circumferential waves, n.
15 Optimal FEM for modal analysis of liquid storage circular tanks 221 Table 2a FE model natural frequencies for empty clamped-free cylindrical tanks (Hz) at different type of shells, 252 No. of Mode m n Experiment Shell 43 Shell 63 Shell 93 Shell 143 Shell 181 Shell 281 FEM (Zienkiewicz [27]) , ,479 1, , , , , , , ,628 1, , , , , , , ,851 1, , , , , , , ,969 2, , , , , , , ,151 2, , , , , , ,
16 222 S.A. Elkholy et al. Table 2b FE model natural frequencies for empty clamped-free cylindrical tanks (Hz) at different type of shells, 448 No. of Mode m n Experiment Shell 43 Shell 63 Shell 93 Shell 143 Shell 181 Shell 281 FEM (Zienkiewicz [27]) , ,479 1, , , , , , , ,628 1, , , , , , , ,851 1, , , , , , , ,969 2, , , , , , , ,151 2, , , , , , ,
17 Optimal FEM for modal analysis of liquid storage circular tanks 223 Table 2c FE model natural frequencies for empty clamped-free cylindrical tanks (Hz) at different type of shells, 1,792 No. of Mode m n Experiment Shell 43 Shell 63 Shell 93 Shell 143 Shell 181 Shell 281 FEM (Zienkiewicz [27]) ,479 1, , , , , , , ,628 1, , , , , , , ,851 1, , , , , , , ,969 2, , , , , , , ,151 2, , , , , , , ,792
18 224 S.A. Elkholy et al. Table 2d FE model natural frequencies for empty clamped-free cylindrical tanks (Hz) at different type of shells, 2,800 No. of Mode m n Experiment SHELL 43 % Difference SHELL163 % Difference SHELL 143 % Difference SHELL181 % Difference FEM % Difference ,479 1, , , , , ,624 1, , , , , ,851 1, , , , , ,969 2, , , , , ,151 2, , , , , ,800
19 Optimal FEM for modal analysis of liquid storage circular tanks 225 Table 2e FE model natural frequencies for empty clamped-free cylindrical tanks (Hz) at different type of shells, 7,168 No. of Mode m n Experiment SHELL 43 % Difference SHELL163 % Difference SHELL181 % Difference FEM % Difference ,479 1, , , , ,624 1, , , , ,851 1, , , , ,969 2, , , , ,151 2, , , , ,168
20 226 S.A. Elkholy et al. Figure 11 Predicted mode shapes for empty shell with different m and n: (a) m = 2, n = 4 (b) m = 2, n = 5 (c) m = 1, n = 5 (d) m = 1, n = 4 (see online version for colours) (a) (b) (c) (d) This table shows that SHELL93 tend to give the least errors which mean that the frequency values predicted by the FE models using these shell are more accurate than the values obtained by using other shell. SHELL 181 yields the highest error, or difference, in all modes between the analytical and experimental results. The other shell give result differences that are more than the result differences produced by SHELL93 and less than the result differences given by SHELL181. It should be noted that SHELL93 (eight-node large strain curved shell) is particularly well suited to analyse empty circular tanks since it is designed model curved shells. Figure 12 shows the effects of the element types on the accuracy of the empty tank natural frequency results by the FE model in comparison with those of experimental measurements. Table 2 and Figures 12 and 13 indicate that no particular SHELL element gives the highest result accuracy for all modes investigated in this paper. However, SHELL with the least result accuracy can be excluded and not recommended for ANSYS FE models used for the analysis of such tanks. It can be seen from Table 2 and Figures 12 and 13 that the option of using SHELL 181 element seems to be the least reliable option in modelling such tanks as it gives the largest difference between the ANSYS FE model results and the experimental values. Therefore, the option of deploying SHELL 181 element in predicting the frequency of the tank will have the least accuracy and should not be recommended. As for increasing the number of in the models, Table 2 shows that for any element used in this study the result differences, in general, decrease as the number of increases leading to a higher accuracy in the FE model output for any mode shape. However, for any mode shape Figures 12 and 13 indicate that as the number of any SHELL element becomes larger the increase in the result accuracy (or the decrease in
21 Optimal FEM for modal analysis of liquid storage circular tanks 227 the % difference) occurs rapidly up to a certain number of after which the accuracy becomes almost steady and almost unaffected by any further increase in the number of. This concludes that increasing the number of is a critical model tuning task and should be carefully sought to get the highest result accuracy with the least model time consumption. Therefore, it should be noted that increasing the element number randomly may not improve the results much but will likely increase the model time consumption. Figure 12 Effect of element types and numbers on the tank natural frequency
22 228 S.A. Elkholy et al. Figure 13 Effect of element numbers (mesh sizes) on the natural frequency (see online version for colours)
23 Optimal FEM for modal analysis of liquid storage circular tanks Full tank case The fluid region is divided into a number of 3-D contained fluid (FLUID80). The fluid movement at the bottom of the tank is considered to be constrained in the vertical direction. The vertical velocities of the fluid element nodes adjacent to each surface of the wetted shell coincide with those of the shell. The boundaries are assumed to be constrained in order to simulate the rigid walls. Figure 14 shows the 3D model of the tank filled with liquid using ANSYS and the shape of the shell meshing. Figure 14 A 3D model of the tank filled with liquid (see online version for colours) The FSI is considered by properly coupling the nodes at the interface of the fluid and the shell in the radial direction. Therefore, the fluid can exert only normal pressure on the tank wall and it can slip on the tank wall in the tangential directions. For the completely filled cylindrical tank, four different idealisations were considered as shown in Table 3. In the first idealisation, a total number of 792 were adopted. In the second idealisation, the number of over the cylindrical shell surface was increased first to 1,792 and then to 3,584. In the final test of idealisation, the number of was increased to 4,480 which were distributed over the shell structure. Figure 15 shows the effects of the element types on the empty tank natural frequency results by the FE model in comparison with those of experimental data. Table 3 and Figures 15 and 16 indicate that most of the shell in any mode shape either have high difference between their outputs and the measured values or have inconsistent behaviour whose result difference increases as the element number increases up to certain element number after which any further increase in the element number will yield a decrease in the difference. In general all of these shell except SHELL43 do not have a unified pattern in all mode shapes. This is attributed to the case studied which is the filled tank case. In this case, FLUID80 (3-D eight-node; with four nodes on each face) are utilised to model the liquid in the curved tank. When a shell element such as SHELL93 (eight-node shell) element or SHELL281 (eight-node shell) element is used to model the curved tank in conjunction with FLUID80 element, this will yield a model whose element nodes are not matching, particularly the mid-span nodes. This will yield inaccurate results. SHELL43 element is the only element among all the investigated in this study which gives the highest result accuracy as it yields consistent results and consistent behaviour patterns in all modes studied. The accuracy of its results increases rapidly as the number of increases up to certain number, after which the accuracy becomes almost steady and almost unaffected by any further increase in the number of. Therefore, SHELL43 seems to be the best and could be recommended for the analysis of filled tank case.
24 230 S.A. Elkholy et al. Table 3a FE model natural frequencies for full clamped-free cylindrical tanks (Hz) with different element numbers, (a) SHELL 43 Mode m n Experiment 792 1, ,027 1, , , , , ,094 1, , , , , ,245 1, , , , , ,299 1, , , , , ,546 1, , , , , ,748 1, , , , , ,584 4,480 Error FEM, [27] Error
25 Optimal FEM for modal analysis of liquid storage circular tanks 231 Table 3b FE model natural frequencies for full clamped-free cylindrical tanks (Hz) with different element numbers, SHELL 63 Mode m n Experiment ,792 3,584 4,480 Error FEM, [27] Error , ,094 1, ,245 1, ,299 1, ,546 1, ,748 1, , , , , , , , , , , , , , , , , , , , , , , ,
26 232 S.A. Elkholy et al. Table 3c FE model natural frequencies for full clamped-free cylindrical tanks (Hz) with different element numbers, SHELL 93 Mode m n Experiment 792 1,792 3,584 4,480 Error FEM, [27] Error , ,094 1, , , , , ,245 1, , , , , ,299 1, Not applicable #VALUE! Not applicable #VALUE! Not applicable #VALUE! 1, ,546 1, , , , , ,748 1, , , , ,
27 Optimal FEM for modal analysis of liquid storage circular tanks 233 Table 3d FE model natural frequencies for full clamped-free cylindrical tanks (Hz) with different element numbers, SHELL 143 Mode m n Experiment ,027 1, ,094 1, ,245 1, ,299 1, ,546 1, ,748 1, ,792 3,584 4,480 Error FEM, [27] Error , , , , , , , , , , , , , , , , , , , , , , ,
28 234 S.A. Elkholy et al. Table 3e FE model natural frequencies for full clamped-free cylindrical tanks (Hz) with different element numbers, SHELL 181 Mode m n Experiment 792 1, ,027 1, , , , , ,094 1, , , , , ,245 1, , , , , ,299 1, , , , , ,546 2, , , , , ,748 2, , , , , ,584 4,480 Error FEM, [27] Error
29 Optimal FEM for modal analysis of liquid storage circular tanks 235 Table 3f FE model natural frequencies for full clamped-free cylindrical tanks (Hz) with different element numbers, SHELL 281 Mode m n Experiment 792 1,792 3,584 4,480 Error FEM, [27] Error , , ,094 1, , , , , ,245 1, , , , , ,299 1, Not applicable #VALUE! Not applicable #VALUE! Not applicable #VALUE! 1, ,546 1, , , , , ,748 1, , , , ,
30 236 S.A. Elkholy et al. Figure 15 Effect of element types and element sizes on the natural frequency (full tank)
31 Optimal FEM for modal analysis of liquid storage circular tanks 237 Figure 16 Effect of element numbers (mesh sizes) on the natural frequency (see online version for colours) 6 Deviation in ANSYS model results Figure 17 shows the average, median, minimum and maximum differences between the experimentally measured frequency values and the model frequency results obtained in this study for both cases of empty tanks and filled tanks. Despite the large deviations between the maximum and minimum differences in both cases, Figure 17 reveals that the median and average difference values are leaning towards the minimum difference values. This indicates that the empty and filled tank frequency values produced in this study by the different ANSYS FE models using different shell and liquid are reasonable and can be described as reliable.
32 238 S.A. Elkholy et al. Figure 17 Deviation in ANSYS model results (see online version for colours) 7 Conclusions and recommendations Empty and liquid filled storage vertical thin tanks are analysed in this paper using ANSYS 3D finite element models. To predict the tank dynamic characteristics such as natural frequencies and principal mode shapes, a number of shell and liquid available in ANSYS element library were utilised extensively. A parametric study of different element numbers for each element type in the 3D FE models was carried out. Tank natural frequencies and mode shapes were obtained and compared with experimentally measured values and analytical results available in the literature. The paper investigated different ANSYS FE 3D models to recommend the optimal element types and element numbers which best predict the empty and filled tank dynamic characteristics of natural frequencies and principal mode shapes. ANSYS, a general-purpose FE programme, element library has many different types of shell six of which were most suitable for modelling the cylindrical tank walls therefore were investigated in this study. These are SHELL43 (four-node plastic large strain shell), SHELL63 (four-node elastic shell), SHELL93 (eight-node large strain curved shell), SHELL143 (eight-node plastic small strain shell) and SHELL181 (four-node finite strain shell) and SHELL281 (eight-node large strain nonlinear shell). As for modelling the fluid in the tank, fluid element FLUID80 (3-D eight-node contained fluid element) was used in this study. To investigate the effects of the element number in the model on the accuracy of the tank calculated dynamic natural frequencies and principal mode shapes, the number of over the cylindrical shell surface was increased gradually from 252 to 7,168. Accordingly, the number of liquid was increased. As it is indicated above, the results of the FE models are greatly influenced by the number of chosen and the meshing scheme utilised. Therefore, to find out the optimal model, it is highly recommended to investigate the optimal number of and corresponding meshing scheme. To fulfil this objective, the analysis should be performed by studying different models with different increasing number of and the optimal model will be the one with the least number of used and that would not cause a significant difference in the results. The study shows that increasing the number of in the radial direction of the tank wall yields a faster increase in the accuracy of the model results than increasing the
33 Optimal FEM for modal analysis of liquid storage circular tanks 239 number of along the height of the tank wall. However, any further increase in the element number beyond a specific element number results in an accuracy that increases at a slower rate and eventually becomes almost steady. For the case of an empty tank, it can be seen from the results obtained in this study that no particular shell element gives the highest result accuracy for all modes. However, SHELL 181 element seems to be the least reliable option in modelling such tanks in all mode shapes as it gives the largest difference between the ANSYS FE model results and the experimental measurements. Therefore, the option of using SHELL 181 element should not be recommended. On the other hand, SHELL93 tend to give the least errors which mean that the frequency values predicted by the FE models using these shell are more accurate than the values obtained by using other shell. SHELL93 element should be recommended for the analysis of empty circular thin tanks as well as structures with similar shapes such as chimneys, shafts and empty circular pipes. As for the number of in the models, the study concludes that increasing the number of is a critical model tuning task and should be carefully selected to get the highest result accuracy with the least model time consumption. The model results indicate that result accuracy increases rapidly as the element number increases but up to a certain number, beyond which the result accuracy becomes almost constant or steady and is not affected by any further increase in the element number in the model. For the case of a filled tank, some shell investigated in this study for any mode shapes have high difference between their results and those of the experimentally measured values. Other have inconsistent results whose difference with the experimental measurements increases as the element number increases in the model up to a certain element number after which any further increase in the element number will yield a decrease in the difference. In general all of these shell, except SHELL43 do not have a unified pattern in all mode shapes. This is attributed to mesh mapping. When a shell element such as SHELL93 (eight-node shell) element or SHELL281 (eight-node shell) element is used to model the curved tank in conjunction with FLUID80 (3-D eight-node with four nodes on each face) element, this will yield a model whose element nodes are not matching, particularly the mid-span nodes. This will yield inaccurate results. SHELL43 element is the only element among all investigated in this study that gives the highest result accuracy as it yields consistent results for all modes. The accuracy of its results increases rapidly as the number of increases up to certain number, after which the accuracy becomes almost steady and unaffected by any further increase in the number of. Therefore, SHELL43 seems to be the best and could be recommended for the analysis of filled tank case. Despite the large deviations between the maximum and minimum differences between the model results and the experimental measurements, the study reveals that the median and average difference values are leaning towards the minimum difference values. This indicates that the empty and filled tank frequency values produced in this study by the different ANSYS FE models using different shell and liquid can be described as reliable. To examine numerically the influence of the element types as well as meshing on the seismic behaviour of real steel tanks, a full-scale tank case and many parameters such as tank configuration, filling ratio and different ground motion characteristics must be considered and highly recommended in future research.
Modelling Flat Spring Performance Using FEA
Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper
More informationNon-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla
Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla 1 Faculty of Civil Engineering, Universiti Teknologi Malaysia, Malaysia redzuan@utm.my Keywords:
More informationCoupled Analysis of FSI
Coupled Analysis of FSI Qin Yin Fan Oct. 11, 2008 Important Key Words Fluid Structure Interface = FSI Computational Fluid Dynamics = CFD Pressure Displacement Analysis = PDA Thermal Stress Analysis = TSA
More informationANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved.
ANSYS Element Selection elearning Peter Barrett October 2012 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection What is the best element type(s) for my analysis? Best
More information17. SEISMIC ANALYSIS MODELING TO SATISFY BUILDING CODES
17. SEISMIC ANALYSIS MODELING TO SATISFY BUILDING CODES The Current Building Codes Use the Terminology: Principal Direction without a Unique Definition 17.1 INTRODUCTION { XE "Building Codes" }Currently
More informationAnalysis of Pile Behaviour due to Damped Vibration by Finite Element Method (FEM)
ISSN 2395-1621 Analysis of Pile Behaviour due to Damped Vibration by Finite Element Method (FEM) #1 L.M.Sardesai, #2 G.A.Kadam 1 sardesaileena@rediffmail.com.com 2 ganeshkadam07@gmail.com #1 Mechanical
More informationAnalysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing
Kasetsart J. (Nat. Sci.) 42 : 165-176 (2008) Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing Chakrit Suvanjumrat*, Tumrong Puttapitukporn and Satjarthip Thusneyapan
More informationGlobal to Local Model Interface for Deepwater Top Tension Risers
Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching
More information2008 International ANSYS Conference
2008 International ANSYS Conference Simulation of Added Mass Effect on Disc Vibrating in Fluid Using Fluid-Structure Interaction Coupling of ANSYS/CFX QIAN LIKE ANSYS Japan K.K. 2008 ANSYS, Inc. All rights
More informationOffshore Platform Fluid Structure Interaction (FSI) Simulation
Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,
More informationCHAPTER 1. Introduction
ME 475: Computer-Aided Design of Structures 1-1 CHAPTER 1 Introduction 1.1 Analysis versus Design 1.2 Basic Steps in Analysis 1.3 What is the Finite Element Method? 1.4 Geometrical Representation, Discretization
More informationChallenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure
Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure In the final year of his engineering degree course a student was introduced to finite element analysis and conducted an assessment
More informationAvailable online at ScienceDirect. Procedia Engineering 111 (2015 )
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 111 (2015 ) 115 120 XXV R-S-P seminar, Theoretical Foundation of Civil Engineering (24RSP) (TFoCE 2015) Numerical simulation
More informationChapter 3 Analysis of Original Steel Post
Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part
More informationA Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections
A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake
More informationApplication of Finite Volume Method for Structural Analysis
Application of Finite Volume Method for Structural Analysis Saeed-Reza Sabbagh-Yazdi and Milad Bayatlou Associate Professor, Civil Engineering Department of KNToosi University of Technology, PostGraduate
More informationSet No. 1 IV B.Tech. I Semester Regular Examinations, November 2010 FINITE ELEMENT METHODS (Mechanical Engineering) Time: 3 Hours Max Marks: 80 Answer any FIVE Questions All Questions carry equal marks
More information3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation
3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack
More informationUsing three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model
Boundary Elements XXVII 245 Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model J. J. Rencis & S. R. Pisani Department of Mechanical Engineering,
More informationSimulation of Sloshing Effects in Cylindrical Containers under Seismic Loading
6. LS-DYNA Anwenderforum, Frankenthal 2007 Bauwesen Simulation of Sloshing Effects in Cylindrical Containers under Seismic Loading Sami A. Kilic 1, Zuhal Ozdemir 2 Assistant Professor 1, Bogazici University,
More informationEffect of Three-Dimensional Geometry on the Sloshing Behavior of Rectangular Concrete Tanks
Effect of Three-Dimensional Geometry on the Sloshing Behavior of Rectangular Concrete Tanks I. Tavakkoli Avval Departmnet of Civil Engineering, Ryerson University, Canada M.R. Kianoush Departmnet of Civil
More informationGuidelines for proper use of Plate elements
Guidelines for proper use of Plate elements In structural analysis using finite element method, the analysis model is created by dividing the entire structure into finite elements. This procedure is known
More informationFinite Element Method. Chapter 7. Practical considerations in FEM modeling
Finite Element Method Chapter 7 Practical considerations in FEM modeling Finite Element Modeling General Consideration The following are some of the difficult tasks (or decisions) that face the engineer
More information2-D Tank Sloshing Using the Coupled Eulerian- LaGrangian (CEL) Capability of Abaqus/Explicit
2-D Tank Sloshing Using the Coupled Eulerian- LaGrangian (CEL) Capability of Abaqus/Explicit Jeff D. Tippmann, Sharat C. Prasad 2, and Parthiv N. Shah ATA Engineering, Inc. San Diego, CA 923 2 Dassault
More informationStudy of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket
RESEARCH ARTICLE OPEN ACCESS Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket Gowtham K L*, Shivashankar R. Srivatsa** *(Department of Mechanical Engineering, B. M.
More informationRevision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction
Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to
More informationCHAPTER 8 FINITE ELEMENT ANALYSIS
If you have any questions about this tutorial, feel free to contact Wenjin Tao (w.tao@mst.edu). CHAPTER 8 FINITE ELEMENT ANALYSIS Finite Element Analysis (FEA) is a practical application of the Finite
More informationStrain-Based Finite Element Analysis of Stiffened Cylindrical Shell Roof
American Journal of Civil Engineering 2017; 5(4): 225-230 http://www.sciencepublishinggroup.com/j/ajce doi: 10.11648/j.ajce.20170504.15 ISSN: 2330-8729 (Print); ISSN: 2330-8737 (Online) Strain-Based Finite
More informationModeling Submerged Structures Loaded by Underwater Explosions with ABAQUS/Explicit
Modeling Submerged Structures Loaded by Underwater Explosions with ABAQUS/Explicit David B. Woyak ABAQUS Solutions Northeast, LLC Abstract: Finite element analysis can be used to predict the transient
More informationSome Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact
Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact Eduardo Luís Gaertner Marcos Giovani Dropa de Bortoli EMBRACO S.A. Abstract A linear elastic model is often not appropriate
More informationA MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun 1
21 st International Conference on Composite Materials Xi an, 20-25 th August 2017 A MODELING METHOD OF CURING DEFORMATION FOR CFRP COMPOSITE STIFFENED PANEL WANG Yang 1, GAO Jubin 1 BO Ma 1 LIU Chuanjun
More informationDesign Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD)
Design Optimization of a Weather Radar Antenna using Finite Element Analysis (FEA) and Computational Fluid Dynamics (CFD) Fernando Prevedello Regis Ataídes Nícolas Spogis Wagner Ortega Guedes Fabiano Armellini
More informationSETTLEMENT OF A CIRCULAR FOOTING ON SAND
1 SETTLEMENT OF A CIRCULAR FOOTING ON SAND In this chapter a first application is considered, namely the settlement of a circular foundation footing on sand. This is the first step in becoming familiar
More informationHydro-elastic analysis of a propeller using CFD and FEM co-simulation
Fifth International Symposium on Marine Propulsors smp 17, Espoo, Finland, June 2017 Hydro-elastic analysis of a propeller using CFD and FEM co-simulation Vesa Nieminen 1 1 VTT Technical Research Centre
More informationCOLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS
VOL., NO., NOVEMBER 6 ISSN 8968 6-6 Asian Research Publishing Network (ARPN). All rights reserved. COLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS
More informationRecent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA
14 th International LS-DYNA Users Conference Session: Simulation Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA Hailong Teng Livermore Software Technology Corp. Abstract This paper
More informationFB-MULTIPIER vs ADINA VALIDATION MODELING
FB-MULTIPIER vs ADINA VALIDATION MODELING 1. INTRODUCTION 1.1 Purpose of FB-MultiPier Validation testing Performing validation of structural analysis software delineates the capabilities and limitations
More informationFluid Structure Interaction - Moving Wall in Still Water
Fluid Structure Interaction - Moving Wall in Still Water Outline 1 Problem description 2 Methodology 2.1 Modelling 2.2 Analysis 3 Finite Element Model 3.1 Project settings 3.2 Units 3.3 Geometry Definition
More informationTechnical Report Example (1) Chartered (CEng) Membership
Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION
More informationModule 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis
25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load
More informationCHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force
CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the
More informationInvestigation of the behaviour of single span reinforced concrete historic bridges by using the finite element method
Structural Studies, Repairs and Maintenance of Heritage Architecture XI 279 Investigation of the behaviour of single span reinforced concrete historic bridges by using the finite element method S. B. Yuksel
More informationElement Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can
TIPS www.ansys.belcan.com 鲁班人 (http://www.lubanren.com/weblog/) Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be
More informationProblem description C L. Tank walls. Water in tank
Problem description A cylindrical water tank is subjected to gravity loading and ground accelerations, as shown in the figures below: Tank walls Water in tank Wall thickness 0.05 C L 5 g=9.81 m/s 2 Water:
More informationFINITE ELEMENT MODELLING AND ANALYSIS OF WORKPIECE-FIXTURE SYSTEM
FINITE ELEMENT MODELLING AND ANALYSIS OF WORKPIECE-FIXTURE SYSTEM N. M. KUMBHAR, G. S. PATIL, S. S. MOHITE & M. A. SUTAR Dept. of Mechanical Engineering, Govt. College of Engineering, Karad, Dist- Satara,
More informationDesign Verification Procedure (DVP) Load Case Analysis of Car Bonnet
Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet Mahesha J 1, Prashanth A S 2 M.Tech Student, Machine Design, Dr. A.I.T, Bangalore, India 1 Asst. Professor, Department of Mechanical
More informationCoustyx Tutorial Indirect Model
Coustyx Tutorial Indirect Model 1 Introduction This tutorial is created to outline the steps required to compute radiated noise from a gearbox housing using Coustyx software. Detailed steps are given on
More informationEngineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering
Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they
More informationDesign procedures of seismic-isolated container crane at port
Design procedures of seismic-isolated container crane at port T.Sugano 1, M.Takenobu 1, T.Suzuki 1, and Y.Shiozaki 2 1 Port and Airport Research Institute,Yokosuka, Japan 2 JFE R&D Corporation,Kawasaki,Japan
More informationRevised Sheet Metal Simulation, J.E. Akin, Rice University
Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.
More informationElfini Solver Verification
Page 1 Elfini Solver Verification Preface Using this Guide Where to Find More Information Conventions What's new User Tasks Static Analysis Cylindrical Roof Under its Own Weight Morley's Problem Twisted
More informationThe Dynamic Response of an Euler-Bernoulli Beam on an Elastic Foundation by Finite Element Analysis using the Exact Stiffness Matrix
Journal of Physics: Conference Series The Dynamic Response of an Euler-Bernoulli Beam on an Elastic Foundation by Finite Element Analysis using the Exact Stiffness Matrix To cite this article: Jeong Soo
More informationSettlement of a circular silo foundation
Engineering manual No. 22 Updated: 02/2018 Settlement of a circular silo foundation Program: FEM File: Demo_manual_22.gmk The objective of this manual is to describe the solution to a circular silo foundation
More informationPerformance of railway track system under harmonic loading by finite element method
Performance of railway track system under harmonic by finite element method Ammar Shuber 1, Mohammed Hamood 1, * and Walaa Jawad 1 1 Building and Construction Engineering Department, University of Technology,
More informationCOMPUTER AIDED ENGINEERING. Part-1
COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.
More informationCHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING
113 CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 6.1 INTRODUCTION Superplastic properties are exhibited only under a narrow range of strain rates. Hence, it
More informationParametric Study of Sloshing Effects in the Primary System of an Isolated LFR Marti Jeltsov, Walter Villanueva, Pavel Kudinov
1 Parametric Study of Sloshing Effects in the Primary System of an Isolated LFR 19.06.2013 Marti Jeltsov, Walter Villanueva, Pavel Kudinov Division of Nuclear Power Safety Royal Institute of Technology
More informationES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010
ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.
More informationWP1 NUMERICAL BENCHMARK INVESTIGATION
WP1 NUMERICAL BENCHMARK INVESTIGATION 1 Table of contents 1 Introduction... 3 2 1 st example: beam under pure bending... 3 2.1 Definition of load application and boundary conditions... 4 2.2 Definition
More informationExample 24 Spring-back
Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static
More informationEmbedded Reinforcements
Embedded Reinforcements Gerd-Jan Schreppers, January 2015 Abstract: This paper explains the concept and application of embedded reinforcements in DIANA. Basic assumptions and definitions, the pre-processing
More informationEXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY
EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY J. Sauvé 1*, M. Dubé 1, F. Dervault 2, G. Corriveau 2 1 Ecole de technologie superieure, Montreal, Canada 2 Airframe stress, Advanced Structures,
More informationVALIDATION OF SASSI2010 SOLUTION METHODS THROUGH INDEPENDENT VERIFICATION USING SAP2000 FOR DEEPLY EMBEDDED STRUCTURES WITH LARGE FOOTPRINTS
Transactions, SMiRT-22 VALIDATION OF SASSI2010 SOLUTION METHODS THROUGH INDEPENDENT VERIFICATION USING SAP2000 FOR DEEPLY EMBEDDED STRUCTURES WITH LARGE FOOTPRINTS Lisa M Anderson 1, Tarek Elkhoraibi,
More informationFinite Element Buckling Analysis Of Stiffened Plates
International Journal of Engineering Research and Development e-issn: 2278-067X, p-issn: 2278-800X, www.ijerd.com Volume 10, Issue 2 (February 2014), PP.79-83 Finite Element Buckling Analysis Of Stiffened
More informationMixed Mode Fracture of Through Cracks In Nuclear Reactor Steam Generator Helical Coil Tube
Journal of Materials Science & Surface Engineering Vol. 3 (4), 2015, pp 298-302 Contents lists available at http://www.jmsse.org/ Journal of Materials Science & Surface Engineering Mixed Mode Fracture
More informationThe part to be analyzed is the bracket from the tutorial of Chapter 3.
Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component
More informationStress Concentration Factors
CONSEIL INTERNATIONAL DES MACHINES A COMBUSTION INTERNATIONAL COUNCIL ON COMBUSTION ENGINES CO-ORDINATING WORKING GROUP "CLASSIFICATION SOCIETIES DIESEL" (WG2) Proposal by CIMAC WG4 11th May 2012 IACS
More information(Based on a paper presented at the 8th International Modal Analysis Conference, Kissimmee, EL 1990.)
Design Optimization of a Vibration Exciter Head Expander Robert S. Ballinger, Anatrol Corporation, Cincinnati, Ohio Edward L. Peterson, MB Dynamics, Inc., Cleveland, Ohio David L Brown, University of Cincinnati,
More informationPrint Depth Prediction in Hot Forming Process with a Reconfigurable Die
Print Depth Prediction in Hot Forming Process with a Reconfigurable Die Jonathan Boisvert* Thibaut Bellizzi* Henri Champliaud Patrice Seers École de Technologie supérieure, Montréal, Québec *Master students,
More informationComputer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks
Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Finite Element Analysis of Bearing Box on SolidWorks Chenling Zheng 1, a, Hang Li 1, b and Jianyong Li 1, c 1 Shandong University
More informationCHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA
DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation
More informationSolid and shell elements
Solid and shell elements Theodore Sussman, Ph.D. ADINA R&D, Inc, 2016 1 Overview 2D and 3D solid elements Types of elements Effects of element distortions Incompatible modes elements u/p elements for incompressible
More informationFigure 30. Degrees of freedom of flat shell elements
Shell finite elements There are three types of shell finite element; 1) flat elements, 2) elements based on the Sanders-Koiter equations and 3) elements based on reduction of a solid element. Flat elements
More informationAIAA Brush Seal Pack Hysteresis
AIAA--3794 Brush Seal Pack Hysteresis Pete F. Crudgington and Aaron Bowsher Cross Manufacturing Co. Ltd Devizes, England Abstract The hysteresis loop that brush seals produce when they are stiffness checked
More informationDr. Sami Kilic Bogazici University. Istanbul, Turkey
Dr. Sami Kilic Bogazici University Dept. of Civil Engineering Istanbul, Turkey Outline Observations about tank damage after the 17 August 1999 Turkish earthquake (Marmara event). Finite element modeling
More informationApplication of a FEA Model for Conformability Calculation of Tip Seal in Compressor
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2008 Application of a FEA Model for Conformability Calculation of Tip Seal in Compressor
More informationSolidWorks. An Overview of SolidWorks and Its Associated Analysis Programs
An Overview of SolidWorks and Its Associated Analysis Programs prepared by Prof. D. Xue University of Calgary SolidWorks - a solid modeling CAD tool. COSMOSWorks - a design analysis system fully integrated
More informationQuarter Symmetry Tank Stress (Draft 4 Oct 24 06)
Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of
More informationME 475 FEA of a Composite Panel
ME 475 FEA of a Composite Panel Objectives: To determine the deflection and stress state of a composite panel subjected to asymmetric loading. Introduction: Composite laminates are composed of thin layers
More informationStress Analysis of thick wall bellows using Finite Element Method
Stress Analysis of thick wall bellows using Finite Element Method Digambar J. Pachpande Post Graduate Student Department of Mechanical Engineering V.J.T.I. Mumbai, India Prof. G. U. Tembhare Assistant
More informationSimulation of Fuel Sloshing Comparative Study
3. LS-DYNA Anwenderforum, Bamberg 2004 Netfreie Verfahren Simulation of Fuel Sloshing Comparative Study Matej Vesenjak 1, Heiner Müllerschön 2, Alexander Hummel 3, Zoran Ren 1 1 University of Maribor,
More informationVerifying finite element model of fixed roof cylindrical liquid container from full scale vibration test results
Verifying finite element model of fixed roof cylindrical liquid container from full scale vibration test results Moslem Amiri, Saeed Reza Sabbagh-Yazdi Civil Engineering Department, K.N. Toosi University
More informationMAE 323: Lab 7. Instructions. Pressure Vessel Alex Grishin MAE 323 Lab Instructions 1
Instructions MAE 323 Lab Instructions 1 Problem Definition Determine how different element types perform for modeling a cylindrical pressure vessel over a wide range of r/t ratios, and how the hoop stress
More informationSTATIC BENDING ANALYSIS OF AN ISOTROPIC CIRCULAR PLATE USING FINITE ELEMENT METHOD
International Journal Modern Trends in Engineering and Research www.ijmter.com e-issn :2349-9745, Date: 28-30 April, 20 STATIC BENDING ANALYSIS OF AN ISOTROPIC CIRCULAR PLATE USING FINITE ELEMENT METHOD
More informationModeling Strategies for Dynamic Finite Element Cask Analyses
Session A Package Analysis: Structural Analysis - Modeling Modeling Strategies for Dynamic Finite Element Cask Analyses Uwe Zencker, Günter Wieser, Linan Qiao, Christian Protz BAM Federal Institute for
More informationIntroduction to the Finite Element Method (3)
Introduction to the Finite Element Method (3) Petr Kabele Czech Technical University in Prague Faculty of Civil Engineering Czech Republic petr.kabele@fsv.cvut.cz people.fsv.cvut.cz/~pkabele 1 Outline
More informationMODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D
MODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D W. Hall, R. P. Jones, and J. T. Mottram School of Engineering, University of Warwick, Coventry, CV4 7AL, UK ABSTRACT: This paper describes a finite element
More informationALE and Fluid-Structure Interaction in LS-DYNA March 2004
ALE and Fluid-Structure Interaction in LS-DYNA March 2004 Workshop Models 1. Taylor bar impact 2. One-dimensional advection test 3. Channel 4. Underwater explosion 5. Bar impacting water surface 6. Sloshing
More informationSimplified modelling of steel frame connections under cyclic loading
Simplified modelling of steel frame connections under cyclic loading Saher El-Khoriby 1), *Mohammed A. Sakr 2), Tarek M. Khalifa 3) and Mohammed Eladly 4) 1), 2), 3), 4) Department of Structural Engineering,
More informationBehaviour of cold bent glass plates during the shaping process
Behaviour of cold bent glass plates during the shaping process Kyriaki G. DATSIOU *, Mauro OVEREND a * Department of Engineering, University of Cambridge Trumpington Street, Cambridge, CB2 1PZ, UK kd365@cam.ac.uk
More informationFINITE ELEMENT MODELLING OF A TURBINE BLADE TO STUDY THE EFFECT OF MULTIPLE CRACKS USING MODAL PARAMETERS
Journal of Engineering Science and Technology Vol. 11, No. 12 (2016) 1758-1770 School of Engineering, Taylor s University FINITE ELEMENT MODELLING OF A TURBINE BLADE TO STUDY THE EFFECT OF MULTIPLE CRACKS
More informationCHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS
CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS 7.1 GENERAL An analytical study on behaviour of combined effect of optimised channel sections using ANSYS was carried out and discussed in
More informationStep Change in Design: Exploring Sixty Stent Design Variations Overnight
Step Change in Design: Exploring Sixty Stent Design Variations Overnight Frank Harewood, Ronan Thornton Medtronic Ireland (Galway) Parkmore Business Park West, Ballybrit, Galway, Ireland frank.harewood@medtronic.com
More informationLab#5 Combined analysis types in ANSYS By C. Daley
Engineering 5003 - Ship Structures I Lab#5 Combined analysis types in ANSYS By C. Daley Overview In this lab we will model a simple pinned column using shell elements. Once again, we will use SpaceClaim
More informationModule 1.6: Distributed Loading of a 2D Cantilever Beam
Module 1.6: Distributed Loading of a 2D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing
More informationEffectiveness of Element Free Galerkin Method over FEM
Effectiveness of Element Free Galerkin Method over FEM Remya C R 1, Suji P 2 1 M Tech Student, Dept. of Civil Engineering, Sri Vellappaly Natesan College of Engineering, Pallickal P O, Mavelikara, Kerala,
More informationCITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1
Outcome 1 The learner can: CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Calculate stresses, strain and deflections in a range of components under
More informationLATERALLY LOADED PILE GROUPS
LATERALLY LOADED PILE GROUPS Pedro Meneses Key words: Group Interaction, Lateral Response, Piles, p-multipliers, p-y Curves. Introduction The lateral resistance of pile foundations is a particularly important
More informationSettlement Analysis of Piled Raft Foundation System (PRFS) in Soft Clay
IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE) e-issn: 2278-1684,p-ISSN: 2320-334X, Volume 14, Issue 2 Ver. VIII (Mar. - Apr. 2017), PP 62-68 www.iosrjournals.org Settlement Analysis of Piled
More informationStudy on Shaking Table Test and Simulation Analysis of Graphite Dowel-Socket Structure
Study on Shaking Table Test and Simulation Analysis of Graphite Dowel-Socket Structure Xiangxiong Kong, Tiehua Shi & Shaoge Cheng Institute of Earthquake Engineering, China Academy of Building Research,
More information