April 23, Abstract
|
|
- Damon Wilson
- 6 years ago
- Views:
Transcription
1 The FCM compared to the h-version FEM for elasto-plastic problems Alireza Abedian 1, Jamshid Parvizian 2, Alexander Düster 3, Ernst Rank 4 (1. Department of Mechanical Engineering, Daneshpajoohan Higher Education Institute, Isfahan, Iran 2. Department of Mechanical Engineering, Isfahan University of Technology, Isfahan, Iran 3. Numerische Strukturanalyse mit Anwendungen in der Schiffstechnik (M-10), Technische Universität Hamburg-Harburg, Hamburg, Germany 4. Lehrstuhl für Computation in Engineering, Fakultät für Bauingenieur- und Vermessungswesen, Technische Universität München, München, Germany) April 23, 2014 Abstract Abstract The Finite Cell Method (FCM) combines the high-order finite element method and the fictitious domain approach for the purpose of simple meshing. In the present study, the FCM is applied to the Prandtl-Reuss flow theory of plasticity and the results are compared with an h-version Finite Element Method (h-fem). The numerical results show that the FCM is more efficient compared to h-fem for elasto-plastic problems, although the mesh does not conform to the boundary. It is also demonstrated that the FCM performs well for elasto-plastic loading and unloading. Key words octree. 1 Introduction Finite Cell Method, h-version Finite Element Method, Prandtl-Reuss, quadtree, The Finite Cell Method (FCM) [1, 2] can be regarded as an embedding or fictitious domain method [3 5], combined with the p-version finite element method [6]. The efficiency of the p-version Finite Element Method (p-fem) for problems of elasto-plasticity has been thoroughly investigated [7 12]; the p-version yields clearly superior accuracy in comparison with its h-version counterparts. Whilst the FCM has been fairly well investigated as an efficient method for linear problems, little has been done to explore its merits in elasto-plastic structural analysis [13 15]. In the FCM, the polynomial degree of the finite element approximation is increased (p-version) to improve the accuracy of the solution, rather than following the traditional mesh refinement approach (h-version). Furthermore, different local refinement strategies have been developed [16,17] for different types of discontinuities and singularities to improve the quality of the FCM approximation. The aim of this paper is to numerically compare the accuracy of the FCM for the Prandtl-Reuss flow theory of plasticity with an h-version FEM. The computations are based on the elasto-plastic J 2 flow theory, using the von Mises yield criterion. Further assumptions include small displacements and small strains. The results show that the FCM makes the analysis of complex geometry problems very convenient and easy as well as reliable. The accuracy of stresses for nearly incompressible materials is always of interest. Incompressibility effects may be introduced by the elasto-plastic material law and may slow down the convergence. The numerical examples Received??.??,?? / Revised??.??,?? Corresponding author Alireza Abedian, Assistant Professor, Ph. D., abedian.a@gmail.com 1
2 presented in this paper demonstrate that a good convergence of stress components can be obtained using FCM, even if the point of interest is located within the plastic region. The paper is organized as follows: Section 2 explains the FCM for elasto-plastic formulation and a modified quadtree integration scheme. Section 3 presents numerical examples used to evaluate the efficiency of the FCM compared to h-fem, for the J 2 plasticity. This is followed by a summary and a conclusion. 2 The Finite Cell Method 2.1 Elasto-plastic formulation The finite cell method is a combination of high-order FEM and fictitious domain methods; we therefore use the well-established terminology of the FEM in this paper. To solve the weak form of the equilibrium equation using the high-order finite cell method, the domain of interest Ω, as shown in Fig. 1, is extended into a domain Ω e, i.e., Ω Ω e, only with the advantage that Ω e can be discretized with a Cartesian structured grid of cells. Ω e \ Ω Ω + = Ω e Figure 1: The domain Ω is extended to Ω e [1]. The weak formulation of the equilibrium conditions of a solid body reads as finding the displacement field u which satisfies the (homogeneous) Dirichlet boundary conditions, so Ω e α ε(v) : σ(u)dω = α v b dω+ v tdγ (1) Ω e Γ N in which b is the vector of volume loads, t is the vector of prescribed tractions on the Neumann boundary Γ N, the operator : denotes the double-contracted product and v is the test function. α is defined as α = { 1.0 in Ω, 0.0 otherwise. (2) In each cell, the displacement field u is approximated using hierarchical shape functions based on integrated Legendre polynomials [18]. Hierarchic bases have been used to implement two different types of Ansatz spaces in two dimensions [6, 19]: the trunk space S p ξ,p η ts (Ω q st ) and the tensor product space S p ξ,p η ps (Ω q st ). Three different types of Ansatz spaces have been implemented in three dimensions [6, 19]: the trunk space S p ξ,p η,p ζ ts (Ω h st ), the tensor product space S p ξ,p η,p ζ ps (Ω h st) and the space S p,p,q (Ω h st). The physically nonlinear problem under contemplation is the J 2 flow theory for small strains with nonlinear isotropic hardening [20]. The strains are small and can be decomposed into an elastic and a plastic component. The stresses should satisfy both the constitutive equations and the equilibrium conditions. Since the nonlinear stress(σ)- strain(ε) relationship depends on the load history, the weak formulation is a nonlinear functional to be solved incrementally. Using the Newton-Raphson method for each step [t (n),t (n+1) ] to linearize the weak formulation, it is 2
3 possible to compute a sequence of equilibrated load steps: Ω e α ε(v) : C (i) (n+1) : ε( u(i+1) )dω = u (i+1) (n+1) α v b (n+1) dω+ v t (n+1) dγ Ω e Γ N α ε(v) : σ (i) (u)dω (3) Ω (n+1) e = u (i) (n+1) + u(i+1) C (i) (n+1) := σ(i) (n+1) ε (i) (n+1) ( ) (i) (n+1) denotes a variable at the ith Newton-Raphson iteration during the load step in[t (n),t (n+1) ]. The actual stress state σ (i) as well as the algorithmic tangent modulus C(i) have to be recomputed at each step i [20]. In linear (n+1) (n+1) elasticity problems the stress(σ)-strain(ε) relationship is linear. The tangent modulus tensor in Equation (3) denotes the elasticity tensor and the equation is solved in one step. The spatial discretization of Equation (3) is performed using the FCM. 2.2 Integration scheme In embedded FE methods, the boundary of the physical domain is not captured by the mesh. Rather, accurate integration schemes may capture the boundary. One of such schemes used for FCM is a modified quadtree integration scheme. Quadtree is a tree data structure used for partitioning a domain by recursively subdividing it into four quadrants. The extension of a quadtree for 3D space is called octree, in which each internal node or domain has eight children [21]. With the help of a quadtree or an octree, it is easy to perform the appropriate numerical integration for Equation (3) using the composed integration over subcells (Fig. 2). η ξ η ξ s r y x Parent cell R = 5 Local coordinate system Figure 2: Composed integration following the relationship of (x, y) and (r, s) for 5 levels of quadtree refinement (R). A mapping has to be applied to establish a relationship between the coordinates of the subcell (r,s) and the cell (ξ, η) [2]. In this investigation, we used a modification of the standard quadtree integration scheme which has two specific features (Fig. 3): (I) Since the subcells are much smaller than the cell, the function over the subcells could be regarded as a lowerorder function; it is accordingly possible to apply low-order Gauss quadrature. In the standard p-fem, p + 1 Gauss points are used in each direction for the elements of order p [8]. We therefore begin with p + 1 Gauss points in each direction; then we reduce the number of Gauss points incrementally down to 1 following the refining of the quadtree. Any integration point outside the boundary of the physical domain defined by the quadtree is ignored. Fig. 3(a) shows the position of active Gauss points of subcells mapped from the local coordinate (r,s) to the parent cell. 3
4 (II) The second feature involves avoiding the ill-conditioning inherent in fictitious methods by assigning a small α to the Gauss points outside the physical domain [1]. Therefore, the cell is reconsidered with p+1 Gauss points in each direction and the points that are outside the physical domain are only taken into account to avoid ill-conditioning of the problem (Fig. 3(b)). As an example, 144 integration points are used for integrating over a cell of order p=4 with 3 levels of quadtree refinement (R = 3), as shown in Fig. 3. η ξ η ξ (a) (b) Figure 3: An adaptive integration scheme consists of a set of integration points inside (a) and outside (b) the physical domain. 3 Numerical examples In each of the examples, the units of dimensions and displacements are in [mm], and stresses in [MPa]. The material is assumed to be elastic/perfectly-plastic with a shear modulus of µ = [MPa], bulk modulus κ = [MPa] and yield stress σ yield = 450 [MPa], [22]. The plane strain situation and a unit thickness are assumed for 2D problems. The computations for FCM are conducted using the p-fem code AdhoC [23], and the direct solver SPOOLES [24] is used to solve the overall equation system. The results are visualised by Paraview [25] using a fine postprocessing mesh. In this paper we will restrict our investigations to a quadtree/octree refinement level of R = 3, and the trunk space S p ξ,p η ts (Ω q st ), S p ξ,p η,p ζ ts (Ω h st ). The FCM leaves the mesh unchanged and progressively increases the degree p, of the piecewise polynomial approximation, until some desired level of precision is reached. In the standard h-fem, however, the mesh is refined and the polynomial degree of the shape functions remains unchanged. The h-version mesh generation and computations were carried out with the commercial finite element package ABAQUS [26] which employs special pressure-displacement elements for incompressible materials, based on a mixed finite element formulation. These elements also include an additional, internal mode trial function [27]. Since it is difficult to create a structured mesh when faced with complex geometries, we made use of the unstructured mesh generating scheme. We chose the 2D and 3D enhanced low-order approximation elements CPE4R (p = 1) and C3D8R (p = 1) in h-fem. The reduced integration scheme and a dense mesh are used to avoid locking and hour-glassing phenomena [27]. 3.1 Perforated plate The first numerical example to be considered is a square plate with a central perforation under cyclic loading. A quarter of the square plate is modelled and the symmetry conditions are imposed on the lower and right sides of the plate (Fig 4). The uniform traction t n = 100 is scaled with a factor 4.5 λ 4.5 in 205 load steps. As a reference solution we use the results provided by Wieners [22] based on a very fine mesh with Q2P1 elements. Results of interest are the stress σ yy at point a=(9,0), the stress σ xx at point b=(6.1953,3.8047), the displacements u x at point c=(0,10) and u y at point d=(10,10). 4
5 The discretization of h-fem and the p-version of the FCM are adjusted to achieve almost the same degrees of freedom (Dofs) for comparison. Fig. 5 shows 100 cells used with p = 10, which corresponds to 9600 Dofs, and 4686 elements of h-fem, which corresponds to 9622 Dofs. t y = λ t n c d λ t n 300 h=10 y x w=10 b a r = 1 load (MPa) load step Figure 4: Perforated square plate under plane strain condition with cyclic loading. Figure 5: Perforated square plate discretized by 100 cells (left) and 4686 elements (right). 5
6 Reference FCM h-fem σyy at point a load factor λ Figure 6: The stress component σ yy at point a Reference FCM h-fem σxx at point b load factor λ Figure 7: The stress component σ xx at point b. 6
7 Reference FCM h-fem ux at point c load factor λ Figure 8: The displacement u x at point c Reference FCM h-fem 0.01 uy at point d load factor λ Figure 9: The displacement u y at point d. As shown in Figs. 6-9, the displacements are approximated accurately by both methods, but the stresses are more accurate using the FCM. Let us consider this problem again with a load factor of λ = 4.5 and study convergence behaviour in terms of Dofs. The first and last mesh used for h-fem are shown in Fig. 10. For FCM calculations, the polynomial degree varies from 4 to 14 using 100 cells (Fig. 5). The results are plotted in the form of relative errors in a double logarithmic scale in Figs. 11 and 12. As these figures indicate, the FCM yields smoother, more accurate results particularly at point a, where the most critical stress concentration occurs. Using FCM, only 4740 Dofs with a corresponding polynomial degree p = 7 are needed to compute the stress components with a relative error less than 7
8 5%. Considering these numerical investigations, it is apparent obvious that it is easy to obtain a degree of accuracy suitable for practical implementation by means of the FCM. Figure 10: Perforated square plate discretized by 777 and 9770 elements. 10 FCM h-fem Relative error [%] 1 5 % relative error 0.1 Dofs Figure 11: Relative error ( σ yy,re f σ yy,fcm σ yy,re f 100[%]) at point a, load factor λ =
9 FCM h-fem Relative error [%] 10 5 % relative error 1 Dofs Figure 12: Relative error ( σ xx,re f σ xx,fcm σ xx,re f 100[%]) at point b, load factor λ = Perforated thick plate For the second example, we consider a thick, perforated plate with a unit thickness under uniform traction of t n = 100 that is raised monotonously to a factor of λ = 4 in 49 load steps (Fig. 13). Symmetry boundary conditions are applied at y = 0,z = 0 and x = 10 planes. By way of a reference solution, we use the p-version FEM with 199 hexahedral elements of p = 10 (Fig. 14), whereas the curved boundary has been represented precisely with blending functions [6]. The result of interest is the stress σ yy at the critical point e= (9,0,0), where the stress concentration occurs. 9
10 t y = λ t n t z y x 400 w λ t n e r h load load step Figure 13: Thick perforated plate under a uniform load. Figure 14: Thick perforated plate discretized by 199 hexahedral elements. 100 cells with p=8 are used for the FCM calculations, which in this case corresponds to Dofs. For the h-version calculations, elements give Dofs (Fig. 15). 10
11 Figure 15: Thick perforated plate discretized using 100 cells and elements. Considering the results in Fig. 16, the FCM approach for p=8 conforms better to the reference solution than the h-fem. It is evident that the FCM provides a more accurate approximation using higher order p. This shows that, the most accurate results can be achieved using FCM σyy at point e Reference FCM h-fem load factor λ Figure 16: The stress component σ yy at point e. A three-dimensional view of the von Mises stress for the FCM with p=8 and the p-version reference solution at the last load step λ = 4 are shown in Fig
12 Figure 17: The von Mises stress results using the FCM (left) and p-version FEM (right) for the last load step λ = 4. Since two different codes, ABAQUS and AdhoC, are used in the present study, it is difficult to achieve a fair comparison for the CPU computational time. It is, however, safe to conclude that it is faster to pursue solution convergence in the FCM, because it has a fixed mesh and the polynomial order is only increased for the sake of a more accurate approximate solution. It is also possible to use a fixed dense pattern of integration points for a p- extension, allowing the entire pre-processing procedure including generating the Cartesian mesh and setting up the integration points to be performed in the beginning of the computation. Besides, the FCM enjoys all the advantages of the p-version FEM, such as condensing interior degrees of freedom which are confined to the element. The elimination of interior degrees of freedom can be performed in parallel on element level without any communication. This increases the efficiency of the overall parallel approach which takes advantage of the fact, that the computation of element matrices of high order constitutes a significant part of the overall numerical effort. Furthermore it can be shown that the elimination of the interior degrees of freedom improves also the conditioning of the resulting global equation system which is important when using iterative solvers [28 31]. 4 Conclusion This paper compared the FCM numerically with an h-version FEM for the Prandtl-Reuss flow theory of plasticity. The results demonstrate the efficiency of the FCM to solve materially nonlinear problems. Numerical examples show that the FCM provides efficient and accurate approximations to this class of physically non-linear problems. It is easier to control the discretization error with the FCM than with the h-fem, so, the degree of error can be reduced by increasing the order of elements and not necessarily by employing a new mesh. Error monitoring and control is achieved automatically, with minimum user interaction and without substantial loss of computational efficiency. For two- and three-dimensional benchmark problems, we find that the models based on the FCM deliver much more accurate results compared with their h-version counterparts. To summarise, the application of the FCM in elastoplastic structural analysis can be recommended. These observations suggest that it would be beneficial to extend the use of the FCM to problems of elastoplasticity with finite strains. Results in this context will be presented in forthcoming papers. 12
13 Acknowledgements This work is the result of an institutional partnership being supported by the Alexander von Humboldt Foundation. This support is gratefully acknowledged. References [1] Parvizian, J., Düster, A. and Rank, E. Finite cell method: h- and p-extension for embedded domain problems in solid mechanics. COMPUT MECH, 41(1), (2007) [2] Düster, A., Parvizian, J., Yang, Z., and Rank, E. The finite cell method for 3D problems of solid mechanics. COMPUT METHOD APPL M, 197, (2008) [3] Saul ev, V. On solving boundary value problems with high performance computers by a fictitious domain method. SIBERIAN MATH J, 4(4), (1963) [4] Neittaanmäki, P. and Tiba, D. An embedding of domains approach in free boundary problems and optimal design. SIAM J CONTROL OPTIM, 33(5), (1995) [5] Rusten, T., Vassilevski, P. and Winther, R. Domain embedding preconditioners for mixed systems. NUMER LINEAR ALGEBR, 5(5), (1998) [6] Szabó, B. and Babuška, I. Finite element analysis, John Wiley & Sons, New York (1991) [7] Düster, A. and Rank, E. A p-version finite element approach for two-and three-dimensional problems of the J 2 flow theory with non-linear isotropic hardening. INT J NUMER METH ENG, 53(1), (2001) [8] Düster, A. and Rank, E. The p-version of the finite element method compared to an adaptive h-version for the deformation theory of plasticity. COMPUT METHOD APPL M, 190(15-17), (2001) [9] Düster, A., Niggl, A., Nübel, V. and Rank, E. A Numerical Investigation of High-Order Finite Elements for Problems of Elastoplasticity. J SCI COMPUT, 17(1), (2002) [10] Holzer, S. and Yosibash, Z. The p-version of the finite element method in incremental elasto-plastic analysis. INT J NUMER METH ENG, 39, (1996) [11] Jeremic, B. and Xenophontos, C. Application of the p-version of the finite element method to elasto-plasticity with localization of deformation.commun NUMER METH EN, 15(12), (1999) [12] Szabó, B., Actis, R. and Holzer, S. Solution of elastic-plastic stress analysis problems by the p-version of the finite element method, Tech. Rep. WU/CCM-93/3, Center for COMPUT MECH, Washington university (1993) [13] Abedian, A., Parvizian, J., Düster, A. and Rank, E. The Finite Cell Method for the J 2 flow theory of plasticity. FINITE ELEM ANAL DES, 69, (2013) [14] Abedian, A., Parvizian, J., Düster, A., Khademyzadeh, H. and Rank, E. Performance of different integration schemes facing discontinuities in the finite cell method. Int J Comput Meth, 10(3), /1-24 (2013). [15] Schillinger, D., Ruess, M., Düster, A. and Rank, E. The Finite Cell Method for large deformation analysis. PAMM, 11, (2011) [16] Joulaian, M. and Düster, A. Local enrichment of the finite cell method for problems with material interfaces. Comput Mech, 52, (2013) [17] Schillinger, D., Düster, A., and Rank, E. The hp-d-adaptive finite cell method for geometrically nonlinear problems of solid mechanics. INT J NUMER METH ENG, 89, (2012) [18] Szabó, B., Düster, A. and Rank, E. The p-version of the Finite Element Method, in: Stein, E., de Borst, R. and Hughes, T. J. R. (Eds.). Encyclopedia of Computational Mechanics, Vol. 1, John Wiley & Sons, Ch. 5, (2004) [19] Düster, A., Bröker, H. and Rank, E. The p-version of the finite element method for three-dimensional curved thin walled structures. INT J NUMER METH ENG, 52, (2001) [20] Simo, J.C. and Hughes, T. J. R. Computational Inelasticity, Springer-Verlag, New York (1998) 13
14 [21] De Berg, M., Cheong, O., Van Kreveld, M. and Overmars, M. Computational geometry: algorithms and applications, Springer-Verlag, New York (2008) [22] Stein, E. Error-controlled adaptive finite elements in solid mechanics, Wiley (2003) [23] Düster, A., Bröker, H., Heidkamp, H., Heißerer, U., Kollmannsberger, S., Krause, R., Muthler, A., Niggl, A., Nübel, V., Rücker, M. and Scholz, D. AdhoC 4 User s Guide, Lehrstuhl für Bauinformatik, Technische Universität München (2004) [24] [25] [26] fea.html [27] Hibbitt, Karlsson, Sorensen, ABAQUS theory manual, Hibbitt, Karlsson & Sorensen (1998) [28] Ainsworth, M. A preconditioner based on domain decomposition for hp-fe approximation on quasi-uniform meshes. SIAM J NUMER ANAL. 33(4), (1996) [29] Mandel, J. Iterative solvers by substructuring for the p-version finite element method. COMPUT METHOD APPL M. 80, (1990) [30] Papadrakakis, M., and Babilis, G., Solution techniques for the p-version of the adaptive fe method. INT J NUMER METH ENG, 37, (1994) [31] Rank, E., Rücker, M., Düster, A., and Bröker, H. The efficiency of the p-version finite element method in a distributed computing environment. INT J NUMER METH ENG. 52, (2001) 14
An immersed boundary approach for the numerical analysis of objects represented by oriented point clouds
An immersed boundary approach for the numerical analysis of objects represented by oriented point clouds László Kudela 1, Stefan Kollmannsberger 1, and Ernst Rank 1,2 1 Chair for Computation in Engineering,
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 informationSmooth finite elements
Smooth finite elements seamless handling of incompressibility, distorted and polygonal meshes; links with equilibrium methods Stéphane Bordas * Nguyen-Xuan Hung ** Nguyen-Dang Hung *** * University of
More informationEffective adaptation of hexahedral mesh using local refinement and error estimation
Key Engineering Materials Vols. 243-244 (2003) pp. 27-32 online at http://www.scientific.net (2003) Trans Tech Publications, Switzerland Online Citation available & since 2003/07/15 Copyright (to be inserted
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 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 informationThe multi-level hp-method for three-dimensional problems: dynamically changing high-order mesh refinement with arbitrary hanging nodes
The multi-level hp-method for three-dimensional problems: dynamically changing high-order mesh refinement with arbitrary hanging nodes Nils Zander 1, Tino Bog 1, Mohamed Elhaddad 1, Felix Frischmann 1,
More informationVisualization of errors of finite element solutions P. Beckers, H.G. Zhong, Ph. Andry Aerospace Department, University of Liege, B-4000 Liege, Belgium
Visualization of errors of finite element solutions P. Beckers, H.G. Zhong, Ph. Andry Aerospace Department, University of Liege, B-4000 Liege, Belgium Abstract The aim of this paper is to show how to use
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 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 informationSmall and large deformation analysis with the p- and B-spline versions of the Finite Cell Method
Noname manuscript No. (will be inserted by the editor) Small and large deformation analysis with the p- and B-spline versions of the Finite Cell Method Dominik Schillinger Martin Ruess Nils Zander Yuri
More informationTo mesh or not to mesh: that is the question
To mesh or not to mesh: that is the question Stefan Kollmannsberger Computation in Engineering Computation in Engineering Ordinarius: Prof. Dr.rer.nat. Ernst Rank Numerical Mechanics: Dr.-Ing. Stefan Kollmannsberger,
More informationNon-Linear Finite Element Methods in Solid Mechanics Attilio Frangi, Politecnico di Milano, February 3, 2017, Lesson 1
Non-Linear Finite Element Methods in Solid Mechanics Attilio Frangi, attilio.frangi@polimi.it Politecnico di Milano, February 3, 2017, Lesson 1 1 Politecnico di Milano, February 3, 2017, Lesson 1 2 Outline
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 informationControl Volume Finite Difference On Adaptive Meshes
Control Volume Finite Difference On Adaptive Meshes Sanjay Kumar Khattri, Gunnar E. Fladmark, Helge K. Dahle Department of Mathematics, University Bergen, Norway. sanjay@mi.uib.no Summary. In this work
More information3D Nearest-Nodes Finite Element Method for Solid Continuum Analysis
Adv. Theor. Appl. Mech., Vol. 1, 2008, no. 3, 131-139 3D Nearest-Nodes Finite Element Method for Solid Continuum Analysis Yunhua Luo Department of Mechanical & Manufacturing Engineering, University of
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 informationTWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS.
Ex_1_2D Plate.doc 1 TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. 1. INTRODUCTION Two-dimensional problem of the theory of elasticity is a particular
More informationMODELLING STIFFENED LIGHTWEIGHT STRUCTURES WITH ISOGEOMETRIC ANALYSIS VIA MORTAR METHODS
ECCOMAS Congress 2016 VII European Congress on Computational Methods in Applied Sciences and Engineering M. Papadrakakis, V. Papadopoulos, G. Stefanou, V. Plevris (eds.) Crete Island, Greece, 5 10 June
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 informationA DESIGN-THROUGH-ANALYSIS APPROACH USING THE FINITE CELL METHOD (ECCOMAS CONGRESS 2016)
ECCOMAS Congress 2016 VII European Congress on Computational Methods in Applied Sciences and Engineering M. Papadrakakis, V. Papadopoulos, G. Stefanou, V. Plevris (eds.) Crete Island, Greece, 5 10 June
More informationHp Generalized FEM and crack surface representation for non-planar 3-D cracks
Hp Generalized FEM and crack surface representation for non-planar 3-D cracks J.P. Pereira, C.A. Duarte, D. Guoy, and X. Jiao August 5, 2008 Department of Civil & Environmental Engineering, University
More informationFigure 1: execution of the program with the definition of the parameters.
The Fortran90 code BEMdyn-incompressible is a general boundary element software suitable to solve problems of incompressible incremental non-linear elasticity with time-harmonic external loads of prescribed
More informationPROPERTIES OF NATURAL ELEMENT COORDINATES ON ANY POLYHEDRON
PROPRTIS OF NATURAL LMNT COORDINATS ON ANY POLYHDRON P. Milbradt and T. Fröbel Institute of Computer Science in Civil ngineering, Univercity of Hanover, 3067, Hanover, Germany; PH (+49) 5-76-5757; FAX
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 informationFinite Volume Methodology for Contact Problems of Linear Elastic Solids
Finite Volume Methodology for Contact Problems of Linear Elastic Solids H. Jasak Computational Dynamics Ltd. Hythe House 200 Shepherds Bush Road London W6 7NY, England E-mail: h.jasak@cd.co.uk H.G. Weller
More informationPATCH TEST OF HEXAHEDRAL ELEMENT
Annual Report of ADVENTURE Project ADV-99- (999) PATCH TEST OF HEXAHEDRAL ELEMENT Yoshikazu ISHIHARA * and Hirohisa NOGUCHI * * Mitsubishi Research Institute, Inc. e-mail: y-ishi@mri.co.jp * Department
More informationCrashbox Tutorial. In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0
Crashbox Tutorial In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0 (Written by Moritz Guenther, student at Altair Engineering GmbH) 1 HyperMesh* 1. Start
More informationCode_Aster. SSND106: Multiple tractions rotations in great deformations, isotropic work hardening
Titre : SSD106 - Tractions rotations multiples en grandes[...] Date : 06/06/2016 Page : 1/9 SSD106: Multiple tractions rotations in great deformations, isotropic work hardening Summary: This test models
More informationAdaptive numerical methods
METRO MEtallurgical TRaining On-line Adaptive numerical methods Arkadiusz Nagórka CzUT Education and Culture Introduction Common steps of finite element computations consists of preprocessing - definition
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 informationVOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL
VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL The following is a description of the model setups and input/output parameters for benchmarking analytical volcanic deformation models
More informationAn explicit feature control approach in structural topology optimization
th World Congress on Structural and Multidisciplinary Optimisation 07 th -2 th, June 205, Sydney Australia An explicit feature control approach in structural topology optimization Weisheng Zhang, Xu Guo
More informationCurved Mesh Generation and Mesh Refinement using Lagrangian Solid Mechanics
Curved Mesh Generation and Mesh Refinement using Lagrangian Solid Mechanics Per-Olof Persson University of California, Berkeley, Berkeley, CA 9472-384, U.S.A. Jaime Peraire Massachusetts Institute of Technology,
More informationFinite Element Analysis Prof. Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology, Madras. Lecture - 36
Finite Element Analysis Prof. Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology, Madras Lecture - 36 In last class, we have derived element equations for two d elasticity problems
More informationExercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method
Exercise 1 3-Point Bending Using the GUI and the Bottom-up-Method Contents Learn how to... 1 Given... 2 Questions... 2 Taking advantage of symmetries... 2 A. Preprocessor (Setting up the Model)... 3 A.1
More informationMetafor FE Software. 2. Operator split. 4. Rezoning methods 5. Contact with friction
ALE simulations ua sus using Metafor eao 1. Introduction 2. Operator split 3. Convection schemes 4. Rezoning methods 5. Contact with friction 1 Introduction EULERIAN FORMALISM Undistorted mesh Ideal for
More informationLarge Rotation Analysis of thin-walled shells
Large Rotation Analysis of thin-walled shells Y. Başar, O. Kintzel Ruhr-University Bochum Bochum, Germany Summary The objective of this contribution is to develop an isoparametric -node shell element by
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 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 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 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 informationCollocation and optimization initialization
Boundary Elements and Other Mesh Reduction Methods XXXVII 55 Collocation and optimization initialization E. J. Kansa 1 & L. Ling 2 1 Convergent Solutions, USA 2 Hong Kong Baptist University, Hong Kong
More informationENGINEERING TRIPOS PART IIA FINITE ELEMENT METHOD
ENGINEERING TRIPOS PART IIA LOCATION: DPO EXPERIMENT 3D7 FINITE ELEMENT METHOD Those who have performed the 3C7 experiment should bring the write-up along to this laboratory Objectives Show that the accuracy
More informationElement Quality Metrics for Higher-Order Bernstein Bézier Elements
Element Quality Metrics for Higher-Order Bernstein Bézier Elements Luke Engvall and John A. Evans Abstract In this note, we review the interpolation theory for curvilinear finite elements originally derived
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 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 information3D NURBS-ENHANCED FINITE ELEMENT METHOD
7th Workshop on Numerical Methods in Applied Science and Engineering (NMASE 8) Vall de Núria, 9 a 11 de enero de 28 c LaCàN, www.lacan-upc.es 3D NURBS-ENHANCED FINITE ELEMENT METHOD R. Sevilla, S. Fernández-Méndez
More informationParallelization of the multi-level hp-adaptive finite cell method
Parallelization of the multi-level hp-adaptive finite cell method John N. Jomo 1, Nils Zander 1, Mohamed Elhaddad 1, Ali Özcan1, Stefan Kollmannsberger 1, Ralf-Peter Mundani 1, and Ernst Rank 1/2 1 Chair
More informationRELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS
International Conference on Economic Engineering and Manufacturing Systems Braşov, 26 27 November 2009 RELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS Galina TODOROVA, Valentin
More informationContents Metal Forming and Machining Processes Review of Stress, Linear Strain and Elastic Stress-Strain Relations 3 Classical Theory of Plasticity
Contents 1 Metal Forming and Machining Processes... 1 1.1 Introduction.. 1 1.2 Metal Forming...... 2 1.2.1 Bulk Metal Forming.... 2 1.2.2 Sheet Metal Forming Processes... 17 1.3 Machining.. 23 1.3.1 Turning......
More informationChapter 7 Practical Considerations in Modeling. Chapter 7 Practical Considerations in Modeling
CIVL 7/8117 1/43 Chapter 7 Learning Objectives To present concepts that should be considered when modeling for a situation by the finite element method, such as aspect ratio, symmetry, natural subdivisions,
More informationDislocation Image Stresses at Free Surfaces by the Finite Element Method
Mat. Res. Soc. Symp. Proc. Vol. 795 2004 Materials Research Society U2.4.1 Dislocation Image Stresses at Free Surfaces by the Finite Element Method Meijie Tang, Guanshui Xu*, Wei Cai, Vasily Bulatov, Lawrence
More informationCoupled analysis of material flow and die deflection in direct aluminum extrusion
Coupled analysis of material flow and die deflection in direct aluminum extrusion W. Assaad and H.J.M.Geijselaers Materials innovation institute, The Netherlands w.assaad@m2i.nl Faculty of Engineering
More informationLarge deformation two- and threedimensional. interfaces using the Finite Cell Method
Faculty of Civil, Geo and Environmental Engineering Chair for Computation in Engineering Prof. Dr. rer. nat. Ernst Rank Large deformation two- and threedimensional contact on embedded interfaces using
More informationContinuum finite element analysis of strain localization in slopes
Continuum finite element analysis of strain localization in slopes Richard A. Regueiro and Ronaldo I. Borja Department of Civil Engineering, Stanford University, USA ABSTRACT: This paper presents a continuum
More informationINTERIOR POINT METHOD BASED CONTACT ALGORITHM FOR STRUCTURAL ANALYSIS OF ELECTRONIC DEVICE MODELS
11th World Congress on Computational Mechanics (WCCM XI) 5th European Conference on Computational Mechanics (ECCM V) 6th European Conference on Computational Fluid Dynamics (ECFD VI) E. Oñate, J. Oliver
More informationThe Finite Element Method for the Analysis of Non-Linear and Dynamic Systems. Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture December, 2013
The Finite Element Method for the Analysis of Non-Linear and Dynamic Systems Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture 11-17 December, 2013 Institute of Structural Engineering Method of Finite Elements
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 informationFinite Element modeling for computational Elastic-Plastic Fracture Mechanics: Crack Tip Opening Displacement (CTOD)
e t International Journal on Emerging Technologies (Special Issue on ICRIET-2016) 7(2): 52-56(2016) ISSN No. (Print) : 0975-8364 ISSN No. (Online) : 2249-3255 Finite Element modeling for computational
More informationWorkshop 15. Single Pass Rolling of a Thick Plate
Introduction Workshop 15 Single Pass Rolling of a Thick Plate Rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for further processing. The rolling process
More informationA Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems
A Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems Yuki ONISHI, Kenji AMAYA Tokyo Institute of Technology
More informationMeshless EPM Solver Technology for Structural Mechanics Problems
A technical note on Meshless EPM Solver Technology for Structural Mechanics Problems by The Computational Mechanic Company, Inc. (COMCO) 7800 Shoal Creek Blvd., Suite 290E Austin, TX 78757 and Altair Engineering
More informationScientific Manual FEM-Design 17.0
Scientific Manual FEM-Design 17. 1.4.6 Calculations considering diaphragms All of the available calculation in FEM-Design can be performed with diaphragms or without diaphragms if the diaphragms were defined
More informationJ. TINSLEY ODEN, and C. ARMANDO DUARTE y. Texas Inst. for Comput. and Appl. Math. The University of Texas at Austin. Taylor Hall 2.
CLOUDS, CRACKS AND FEM'S J. TINSLEY ODEN, and C. ARMANDO DUARTE y Texas Inst. for Comput. and Appl. Math. The University of Texas at Austin Taylor Hall 2.400 Austin, Texas, 78712, U.S.A. Dedicated to Professor
More informationENHANCED STRUCTURE CAE SOLUTION WITH MOLDING EFFECT FOR AUTOMOTIVE PARTS
ENHANCED STRUCTURE CAE SOLUTION WITH MOLDING EFFECT FOR AUTOMOTIVE PARTS Allen Y. Peng*, Wen-Hsien Yang, David C. Hsu CoreTech System Co., Ltd., HsinChu, Taiwan, ROC Abstract An increasing number of automotive
More informationAdvanced Professional Training
Advanced Professional Training Non Linea rand Stability All information in this document is subject to modification without prior notice. No part of this manual may be reproduced, stored in a database
More informationTHE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT
Journal of MECHANICAL ENGINEERING Strojnícky časopis, VOL 67 (2017), NO 2, 69-76 THE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT OPLT Tomáš 1,2, POKORNÝ Pavel 2,
More informationLOCAL STRESS ANALYSIS OF STIFFENED SHELLS USING MSC/NASTRAN S SHELL AND BEAM p-elements
LOCAL STRESS ANALYSIS OF STIFFENED SHELLS USING MSC/NASTRAN S SHELL AND BEAM p-elements Sanjay Patel, Claus Hoff, Mark Gwillim The MacNeal-Schwendler Corporation Abstract In large finite element models
More informationThe weak substitution method An application of the mortar method for patch coupling in NURBS-based isogeometric analysis
The weak substitution method An application of the mortar method for patch coupling in NURBS-based isogeometric analysis W. Dornisch, G. Vitucci, S. Klinkel Lehrstuhl für Baustatik und Baudynamik, RWTH
More informationAdaptive Isogeometric Analysis by Local h-refinement with T-splines
Adaptive Isogeometric Analysis by Local h-refinement with T-splines Michael Dörfel 1, Bert Jüttler 2, Bernd Simeon 1 1 TU Munich, Germany 2 JKU Linz, Austria SIMAI, Minisymposium M13 Outline Preliminaries:
More informationDepartment of Computing and Software
Department of Computing and Software Faculty of Engineering McMaster University Assessment of two a posteriori error estimators for steady-state flow problems by A. H. ElSheikh, S.E. Chidiac and W. S.
More informationTICAM - Texas Institute for Computational and Applied Mathematics. The University of Texas at Austin. Taylor Hall Abstract
A New Cloud-Based hp Finite Element Method J. T. Oden, C. A. M. Duarte y and O. C. Zienkiewicz z TICAM - Texas Institute for Computational and Applied Mathematics The University of Texas at Austin Taylor
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 informationABAQUS for CATIA V5 Tutorials
ABAQUS for CATIA V5 Tutorials AFC V2.5 Nader G. Zamani University of Windsor Shuvra Das University of Detroit Mercy SDC PUBLICATIONS Schroff Development Corporation www.schroff.com ABAQUS for CATIA V5,
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 informationCONTACT STATE AND STRESS ANALYSIS IN A KEY JOINT BY FEM
PERJODICA POLYTECHNICA SER. ME CH. ENG. VOL. 36, NO. 1, PP. -15-60 (1992) CONTACT STATE AND STRESS ANALYSIS IN A KEY JOINT BY FEM K. VARADI and D. M. VERGHESE Institute of Machine Design Technical University,
More informationGenerative Part Structural Analysis Fundamentals
CATIA V5 Training Foils Generative Part Structural Analysis Fundamentals Version 5 Release 19 September 2008 EDU_CAT_EN_GPF_FI_V5R19 About this course Objectives of the course Upon completion of this course
More informationIdentification of strain-rate sensitivity parameters of steel sheet by genetic algorithm optimisation
High Performance Structures and Materials III Identification of strain-rate sensitivity parameters of steel sheet by genetic algorithm optimisation G. Belingardi, G. Chiandussi & A. Ibba Dipartimento di
More information13.472J/1.128J/2.158J/16.940J COMPUTATIONAL GEOMETRY
13.472J/1.128J/2.158J/16.940J COMPUTATIONAL GEOMETRY Lecture 23 Dr. W. Cho Prof. N. M. Patrikalakis Copyright c 2003 Massachusetts Institute of Technology Contents 23 F.E. and B.E. Meshing Algorithms 2
More informationDetermination of the solicitation types responsible for the deformed. shape of an aircraft cockpit
Determination of the solicitation types responsible for the deformed shape of an aircraft cockpit Infante, V. 1*, Gomes, E. 1 and Branco, C.M. 1 1 Departamento de Engenharia Mecânica, Instituto Superior
More informationFinite element algorithm with adaptive quadtree-octree mesh refinement
ANZIAM J. 46 (E) ppc15 C28, 2005 C15 Finite element algorithm with adaptive quadtree-octree mesh refinement G. P. Nikishkov (Received 18 October 2004; revised 24 January 2005) Abstract Certain difficulties
More informationContents. I The Basic Framework for Stationary Problems 1
page v Preface xiii I The Basic Framework for Stationary Problems 1 1 Some model PDEs 3 1.1 Laplace s equation; elliptic BVPs... 3 1.1.1 Physical experiments modeled by Laplace s equation... 5 1.2 Other
More informationSimilar Pulley Wheel Description J.E. Akin, Rice University
Similar Pulley Wheel Description J.E. Akin, Rice University The SolidWorks simulation tutorial on the analysis of an assembly suggested noting another type of boundary condition that is not illustrated
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 informationANSYS Workbench Guide
ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through
More informationNumerical simulation of CAD thin structures using the extended Finite Element Method and Level Sets
Numerical simulation of CAD thin structures using the extended Finite Element Method and Level Sets G. Legrain a,, C. Geuzaine b, J.F. Remacle c, N. Moës a, P. Cresta d, J. Gaudin e a LUNAM Université,
More information1. Carlos A. Felippa, Introduction to Finite Element Methods,
Chapter Finite Element Methods In this chapter we will consider how one can model the deformation of solid objects under the influence of external (and possibly internal) forces. As we shall see, the coupled
More informationLevel-set and ALE Based Topology Optimization Using Nonlinear Programming
10 th World Congress on Structural and Multidisciplinary Optimization May 19-24, 2013, Orlando, Florida, USA Level-set and ALE Based Topology Optimization Using Nonlinear Programming Shintaro Yamasaki
More informationSimulation of Lamb waves using the spectral cell method
Simulation of Lamb waves using the spectral cell method S. Duczek a, M. Joulaian b, A. Düster b and U. Gabbert a a Otto-von-Guericke-University Magdeburg, Universitätsplatz 2, 39106 Magdeburg, Germany;
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 informationCSMA A scalable implementation of a volume coupling scheme for the modeling of polycrystalline materials. 1 Motivation
A scalable implementation of a volume coupling scheme for the modeling of polycrystalline materials T. Milanetto Schlittler, R. Cottereau 2 CSMA 207 3ème Colloque National en Calcul des Structures 5-9
More informationHigh Order Nédélec Elements with local complete sequence properties
High Order Nédélec Elements with local complete sequence properties Joachim Schöberl and Sabine Zaglmayr Institute for Computational Mathematics, Johannes Kepler University Linz, Austria E-mail: {js,sz}@jku.at
More informationNumerical simulation of tunnel construction in volcanic rocks
Numerical simulation of tunnel construction in volcanic rocks G. Beer, Ch. Duenser Graz University of Technology, Graz, Austria ABSTRACT: For the design of tunnels, numerical simulation plays an important
More informationMODELING MIXED BOUNDARY PROBLEMS WITH THE COMPLEX VARIABLE BOUNDARY ELEMENT METHOD (CVBEM) USING MATLAB AND MATHEMATICA
A. N. Johnson et al., Int. J. Comp. Meth. and Exp. Meas., Vol. 3, No. 3 (2015) 269 278 MODELING MIXED BOUNDARY PROBLEMS WITH THE COMPLEX VARIABLE BOUNDARY ELEMENT METHOD (CVBEM) USING MATLAB AND MATHEMATICA
More informationX-FEM based modelling of complex mixed mode fatigue crack propagation
X-FEM based modelling of complex mixed mode fatigue crack propagation Hans Minnebo 1, Simon André 2, Marc Duflot 1, Thomas Pardoen 2, Eric Wyart 1 1 Cenaero, Rue des Frères Wright 29, 6041 Gosselies, Belgium
More informationTruss structural configuration optimization using the linear extended interior penalty function method
ANZIAM J. 46 (E) pp.c1311 C1326, 2006 C1311 Truss structural configuration optimization using the linear extended interior penalty function method Wahyu Kuntjoro Jamaluddin Mahmud (Received 25 October
More informationA new 8-node quadrilateral spline finite element
Journal of Computational and Applied Mathematics 195 (2006) 54 65 www.elsevier.com/locate/cam A new 8-node quadrilateral spline finite element Chong-Jun Li, Ren-Hong Wang Institute of Mathematical Sciences,
More informationStress analysis of toroidal shell
Stress analysis of toroidal shell Cristian PURDEL*, Marcel STERE** *Corresponding author Department of Aerospace Structures INCAS - National Institute for Aerospace Research Elie Carafoli Bdul Iuliu Maniu
More information