Finite-element method (FEM) - 190

Application

Virtually all technical procedures can be simulated on a computer with the finite-element method FEM (the term having been introduced by Ray W. Clough at the start of the 1960s [1]). However, this involves breaking down any body (gaseous, liquid, or solid) into elements that are simple in shape (line, triangle, square, tetrahedron, pentahedron, or hexahedron), that are as small as possible, and that are permanently connected to each other at their corner points (“nodes”). Small elements are important because the behavior of elements formulated by approximation using linear equations is only applicable to infinitesimal elements. However, the computing time calls for finite elements. The approximation to reality is better the smaller the elements are. The application of FEM in practice – also known as FEA (finite-element analysis) – began in the early 1960s in the aviation and aerospace industries and followed soon after in automobile manufacturing. Today the method is used in all fields of technology, including weather forecasting, medical science, and for many sectors of automobile manufacturing ranging from engine and chassis components through to body calculations and crash behavior. There are two different types of application. Firstly, virtually fully automatic “Black Box” FEM contained in all CAD programs (computer-aided design) for rough calculations by the design engineer (e.g. in designing a bumper) and, secondly, the use reserved for specialists of special FEM programs (e.g. in body calculations, in axle development or in driving dynamics).

 

FEM program system

The software of an FEM system consists of a preprocessor, a postprocessor, and the actual FEM program. Network creation, i.e. breakdown into elements, is mainly performed in the preprocessor on the basis of a CAD geometry which is read directly or via neutral interfaces such as IGES (Initial Graphics Exchange Specification)

VDA-FS (Verband der Automobilindustrie – Flächenschnittstelle) or STEP (Standard for the Exchange of Product Model Data). The FEM program calculates the computing model formulated in this way. The result found is then shown in graphic form in the postprocessor (e.g. stress distribution by means of isocolors, deformations as motion animation).

 

Basic knowledge for application

FEM is, like all numerical methods, an approximation process. In mechanics, the main area of application, the limitations caused by this are described in the following. Small motions in one solution step Bodies move on paths which are normally higher-order curves. With the basic principle of linearization of all processes, this motion is limited to a straight path which can then be described by linear equations. When transferred to the element corners (nodes), they also move on a straight line. Thus, the nodes are only able to realize very small motions correctly (node twists less than 3.5°). The actual motion along any path or nonlinear material behavior is thus solved linearly with many small steps. Calculation accuracy The linear equation system is formulated and solved with the limited computing accuracy of a computer. Usually, 8 bytes (=  64 bits) are used with a computing accuracy of 13 significant digits for the number stored, i.e. only the first 13 digits of a number can be represented exactly. The further digits in this number are random numbers. As a result, this rules out the possibility of any stiffness differences of the individual components in a model. Therefore, in the deformation calculation of a body, it is necessary, as for example in the measurement of body deformation, to replace the axle springs with rigid supports.

Interpretation of results The great danger lies in the fact that a formal computation model formulated correctly by a beginner will indeed deliver beautifully colorful images, but the results shown can center around factors far from reality. The problems resulting from the abovementioned limitations must therefore be identified and signaled by the computing program, so that the less experienced user is also able to obtain correct results easily

 

Areas of FEM application

In technology terms, physics is generally divided into five areas – mechanics with statics and kinematics (e.g. body, axle), dynamics with acoustics (e.g. vehicle noise), thermodynamics (e.g. temperature distribution in the engine), electricity with magnetism (e.g. ignition coil, sensor technology), and optics (e.g. headlamp). When it comes to FEM, a distinction is always made between – linear and nonlinear static and dynamic problems with the deformations as an unknown for stress calculation and dynamic analysis, – stationary (timeless) and nonstationary (time-dependent) potential problems (e.g. temperature, sound pressure, electrical or magnetic potential) with the potentials as an unknown, – and the linking of these different fields, e.g. to calculate a temperature field and the resulting deformations, stresses and forces in linear statics when the engine is started

 

Elements of FEM

The properties of the elements define the most important performance data of an FEM program. The element quality is determined by the degree of the mathematical formulation function selected. Here, for example, a distinction is made between elements with a linear or quadratic formulation, recognizable from the midside node in the middle of the edge. The quality of a computing model is therefore dependent not just on the fineness of the used mesh, but also quite considerably on the formulation function. A distinction is made between three different types of elements: line elements, shell elements, and volume elements. Line elements Line elements (Figure 1) are either straight or curved with an midside node. The cross-sections are described by specifying the numerical values for the cross-sectional area A, the reduced shear cross-sections Ared-v-w (shear areas), the principal moments of inertia (Iv, Iw), the torsional moment of inertia (It) with the torsional section modulus (Wt), the sector moment of inertia for warping-force torsion, an angle α which describes the position of principal axes of inertia υ and w in relation to the road plane, and the maximum four stress points (Sv, Sw) for bending-stress calculation. Shell elements Shell elements (Figure 2) are either triangular or quadrangular in shape – ideally an equilateral triangle or a square, usually of constant thickness. If the midside nodes are omitted, the edges are straight.

 

Volume (solid) elements

Volume elements (Figure 3) as tetrahedrons, pentahedrons and hexahedrons without midside nodes have straight edges – ideally an equilateral tetrahedron or a cube. With a sufficient number of elements in relation to the thickness (greater than or equal to three), elements with midside nodes are not necessary today. However, this does not apply to tetrahedrons, which are almost alway used in the case of a complicated geometry, such as a cylinder head for example.

 

Modeling and evaluation of results The most important function in using an FEM program is the usually time-consuming task of creating the input data as a computing model with the preprocessor. The user should try to achieve this target with as few elements and nodes as possible (however, the computing model of a body today has approximately three to four million nodes). To do so, the user requires a certain level of experience, but must have an exact knowledge of the qualities of the elements used (see FEM examples). These can differ slightly in every FEM program. The first step in modeling involves choosing the element type (line, shell or volume element) and determining the fineness of the mesh, e.g. by means of the specified middle element-edge length. The next step involves defining the properties (material data), e.g. the element thickness for unit elements, the cross-section values for line elements, and the units used (e.g. length in mm and force in N). A further step involves determining support conditions and load. The crucial factor here is considering the points where a model is fixed, and where it is loaded. In relation to loading, it is also useful to conduct a breakdown of the total load into load cases, e.g. into the mass load from gravity weight and different traffic loads. All FEM results are available in list form or postprocessor data format, and can therefore be shown in graphic form (see FEM examples). To this end, the postprocessor offers all the conceivable forms of display.

 

FEM examples

For the examples, modeling is performed on the basis of CAD geometry using the FEM program TP2000. The model inputs, together with color representation of the results, can also be found on the Internet page specified in [2]. In reality, all bodies are three-dimensional. In simulation, a simplified solution is often chosen in order to save time and expense. It is much easier, for example, to realize the automatic meshing of a flat surface in shell elements than it is to realize a body in its volume elements. The frequently used tetrahedron mesh, which today every preprocessor creates for any volume geometry, does not always live up to expectations. In automobile manufacturing, the structural components are either thick-walled and solid (e.g. engine, transmission, axles, wheels) and modeled with volume elements or they are made from thin-walled sheet metal (e.g. automobile body, truck cab) and are modeled with shell and line elements. The first example, as a volume-element model, belongs to the first group of thickwalled, solid components. It is compared with the commonly used shell model of the second group. This also includes the line element commonly used in automobile manufacturing with the second example

Example 1: Cast-steel engine mount as shell- and volume-element model (linear statics) The aim is to compare shell and volume elements in linear statics on a relatively thick-walled (3.75 mm) cast-steel engine mount (50 × 25 × 57 mm3 ). In the volume elements, two models A and B (each with and without midside nodes) with significantly different result qualities are compared; added to this is shell model C (Figure 4). Starting out from the CAD volume geometry, the preprocessor automatically creates volume-element networks A and B, and also shell-element model C by means of the surface model. The material properties in the units mm, N and kg are: Modulus of elasticity: 210,000 N/mm2 Poisson’s ratio: 0.3 Density: 0.00000785 kg/mm3 . In the case of models A and B, the element properties are defined with the element type “Solid” (volume) with three node degrees of freedom υx, υy and υz. In the case of model C, the properties are defined with the element type “Plate” (shell) with six node degrees of freedom υx, υy, υz, dx, dy, dz and constant thickness d = 3.75 mm. In model A, the meshing with volume elements (solid mesh) shows the preferred breakdown into hexahedrons (not possible fully automated for all geometries because here, for example, the geometry first had to be broken down into basic bodies) and in model B, the automatic tetrahedron meshing. The number of elements in relation to thickness which is crucial for accuracy is specified (at least three elements here). Support conditions On the rectangular xz plane, υy = 0 applies to all nodes. All the edge nodes on the right long leg are pinned by υx = 0, and those of the lower short leg are pinned by υz = 0. Loading ∑Fx =900 N, ∑Fy =2006 N, ∑Fz =−550 N. All the loads are defined as surface load (“on surface”, for shell “on curve”) at the recess at Fx = 600 N, at the small hole at Fy=2006 N, and at the large hole at Fz = −550 N. Note: “Isolated” individual loads are only permitted with line elements. Result The results are shown in Table 1. Figure 5 shows the result for model A with stresses as shades of gray (critical areas are shown in dark) or as isocolors in the original. Volume elements are very sensitive to incorrectly approximated load distributions. Volume elements should therefore only ever be subjected to surface loads. Considering Table 1 in detail: Experience shows that model A2 with midside nodes delivers the correct result (υ = 0.064 mm, σ = 195  MPa). The deviation between averaged and maximum node stress (from all the elements at the same node) should be as small as possible (less than 15 %). This is achieved with model A1 at 11 % with three elements per thickness. In model B1 with three tetrahedrons per thickness, the deformation is 25 % too small (υ = 0.048 mm), and the maximum stress is also 25 %. With only two tetrahedrons in relation to the thickness, the model would even be 58 % too rigid and can barely be used with correspondingly lower stresses. However, with midside nodes (B2), it delivers virtually identical deformations and stresses to A2 with a very large number of nodes and long computing times. Caution is therefore advised with rough tetrahedron mesh without midside nodes.

Model C with shell elements without shear deformation (only intended for thin-walled structures) is clearly too soft (υ = 0.081 mm, 21 % greater, as thickwalled with shear deformation even 30 % greater). Shell elements, whether thin- or thick-walled, deliver only partially usable deformations with relatively large thickness, particularly in the case of very compact bodies, as is the case here. However, at stresses of +14 %, it is for the most part on the safe side.