• Corpus ID: 53462539

Reliable FE-Modeling with ANSYS

@inproceedings{Nelson2004ReliableFW,
  title={Reliable FE-Modeling with ANSYS},
  author={Thomas Nelson and Erke Wang},
  year={2004}
}

• T. Nelson, Erke Wang
• Published 2004
• Computer Science

ANSYS is one of the leading commercial finite element programs in the world and can be applied to a large number of applications in engineering. Finite element solutions are available for several engineering disciplines like statics, dynamics, heat flow, fluid flow, electromagnetics and also coupled field problems. It is well known that a finite element solution is always an approximate solution of the considered problem and one always has to decide whether it is a good or a bad solution. Hence, the question is how a finite element solution can be validated. In this paper we mention several aspects of modelling to obtain a good finite element solution for problems in structural mechanics. Although ANSYS gives quite a lot of warnings to prevent the user from making modelling mistakes, there are still some aspects during the preand postprocessing and also during the solution process we would like to discuss just to point out where user knowledge might still be necessary to obtain good results. In our investigations we use both ANSYS products: ANSYS and ANSYS Workbench. Several ways of modelling a problem of structural mechanics are discussed, taking into account the different available features of ANSYS and ANSYS Workbench. Introduction The finite element method (FEM) is the most popular simulation method to predict the physical behaviour of systems and structures. Since analytical solutions are in general not available for most daily problems in engineering sciences numerical methods have been evolved to find a solution for the governing equations of the individual problem. Although the finite element method was originally developed to find a solution for problems of structural mechanics it can nowadays be applied to a large number of engineering disciplines in which the physical description results in a mathematical formulation with some typical differential equations which can be solved numerically. Much research work has been done in the field of numerical modelling during the last thirty years which enables engineers today to perform simulations close to reality. Nonlinear phenomena in structural mechanics such as nonlinear material behaviour, large deformations or contact problems have become standard modelling tasks. Because of a rapid development in the hardware sector resulting in more and more powerful processors together with decreasing costs of memory it is nowadays possible to perform simulations even for models with millions of degrees of freedom. In a mathematical sense the finite element solution always just gives one an approximate numerical solution of the considered problem. Sometimes it is not always an easy task for an engineer to decide whether the obtained solution is a good or a bad one. If experimental or analytical results are available it is easily possible to verify any finite element result. However, to predict any structural behaviour in a reliable way without experiments every user of a finite element package should have a certain background about the finite element method in general. In addition, he should have fundamental knowledge about the applied software to be able to judge the appropriateness of the chosen elements and algorithms. This paper is intended to show a summary of ANSYS capabilities to obtain results of finite element analyses as accurate as possible. Many features of ANSYS are shown and where it is possible we show what is already implemented in ANSYS Workbench. We will distinguish two different sources of errors within a finite element analysis. On the one hand some mistakes might be introduced in the analysis because the user himself does not know enough about finite elements in general. To minimize these errors we summarize important features of certain element types and element formulations of ANSYS. We also discuss the quality of different element shapes with respect to accuracy and finally provide some information of a correct coupling of different element types. On the other hand errors might occur due to a poor quality of the used finite element program itself. A high-quality program assists the user in reporting reasonable warnings and errors. We will discuss some typical error messages from ANSYS, which allow the user to correct a finite element model immediately. Some reasons possibly leading to poor finite element results are summarized in Tab.1 below to give a coarse overview: Table 1: Possible sources of errors in a finite element analysis Engineer Finite Element Software wrong element type bad element formulation Preprocessing wrong element coupling bad meshing algorithm wrong idealization no warnings and errors wrong calculation discipline wrong calculation algorithm Solution wrong boundary conditions inaccurate equilibrium iteration wrong convergence criteria no warnings and errors wrong result coordinate system wrong result averaging Postprocessing wrong selection of components wrong displaying of results wrong interpolation of results no warnings and errors We should not forget to point out, that ANSYS is a general purpose program, where many numerical modelling techniques are implemented. However, it is sometimes not easy to learn especially for beginners or even for designers, who are usually not finite element experts. With ANSYS Workbench some effort has been done to offer a product, which has implemented by default the best algorithms of ANSYS and is furthermore very easy to use. Hence we will always discuss in this paper as a first step some modelling features of ANSYS and finally point out which of them are already available in ANSYS Workbench. Preprocessing First of all, we will summarize some important aspects every user should be familiar with when doing the preprocessing of a finite element analysis with ANSYS. The following topics will be discussed very briefly: consequences of different element shape functions, important features of different beam and shell elements, results of different element shapes and element formulations and finally correct coupling of different element types. In addition to that, we show what kind of help is available from ANSYS in terms of warnings and errors during the preprocessing to minimize modelling mistakes. User knowledge during preprocessing Choosing an element with linear or a quadratic shape functions To make it as easy as possible we will just look at elements with displacement degrees of freedom – no rotational degrees of freedom are present. In ANSYS such elements are called SOLID... (acting in 3D), PLANE...(acting in 2D) or LINK... (acting in 1D), respectively. Let us consider the one-dimensional case. Within one element the displacements are supposed to vary in a linear or quadratic manner: x a a x u ⋅ + = 1 0 ) ( (1) 2 2 1 0 ) ( x a x a a x u ⋅ + ⋅ + = (2) Hence, we talk about linear or quadratic elements. As a consequence of that assumption the strain and also the stress distribution is either constant or linear within each element due to: dx du x = ) ( ε and ) ( ) ( x E x ε σ ⋅ = (3) This may be easily illustrated in the following one-dimensional truss example. The resulting displacement and stress distribution is shown for a two element discretization with linear and quadratic elements: Figure 1. One dimensional truss problem: linear and quadratic elements and their consequences With E as Young’s Modulus, F as applied force, and A(x) as the cross sectional area the analytic solution is dx x A E F x u x ∫ = 0 ) ( 1 ) ( and ) ( ) ( x A F x = σ (4) coming from a direct integration of the governing differential equation of the above considered problem. It is generally known that better results can be obtained using the same discretization with quadratic or higher order elements compared with the results of linear or lower order elements. You should also keep in mind that the degree of freedom solution always shows a smooth distribution from element to element whereas the distribution of derived quantities (such as strains and stresses) is no longer smooth at the element boundaries. This is a correct result in terms of the finite element method. Just the so-called “weak formulation” of the concerning differential equation is solved by finite elements and the continuity requirements for the governing variables of the problem are relaxed. F