김경종
349 lines
27 KiB
Markdown
349 lines
27 KiB
Markdown
<!-- source-page: 21 -->
|
||
|
||
predicted, and it is most important to select mathematical models that are reliable and effective in predicting the quantities sought.
|
||
|
||
To define the reliability and effectiveness of a chosen model we think of a very-comprehensive mathematical model of the physical problem and measure the response of our chosen model against the response of the comprehensive model. In general, the very-comprehensive mathematical model is a fully three-dimensional description that also includes nonlinear effects.
|
||
|
||
# Effectiveness of a mathematical model
|
||
|
||
The most effective mathematical model for the analysis is surely that one which yields the required response to a sufficient accuracy and at least cost.
|
||
|
||
# Reliability of a mathematical model
|
||
|
||
The chosen mathematical model is reliable if the required response is known to be predicted within a selected level of accuracy measured on the response of the very-comprehensive mathematical model.
|
||
|
||
Hence to assess the results obtained by the solution of a chosen mathematical model, it may be necessary to also solve higher-order mathematical models, and we may well think of (but of course not necessarily solve) a sequence of mathematical models that include increasingly more complex effects. For example, a beam structure (using engineering terminology) may first be analyzed using Bernoulli beam theory, then Timoshenko beam theory, then two-dimensional plane stress theory, and finally using a fully three-dimensional continuum model, and in each case nonlinear effects may be included. Such a sequence of models is referred to as a hierarchy of models (see K. J. Bathe, N. S. Lee, and M. L. Bucalem [A]). Clearly, with these hierarchical models the analysis will include ever more complex response effects but will also lead to increasingly more costly solutions. As is well known, a fully three-dimensional analysis is about an order of magnitude more expensive (in computer resources and engineering time used) than a two-dimensional solution.
|
||
|
||
Let us consider a simple example to illustrate these ideas.
|
||
|
||
Figure 1.2(a) shows a bracket used to support a vertical load. For the analysis, we need to choose a mathematical model. This choice must clearly depend on what phenomena are to be predicted and on the geometry, material properties, loading, and support conditions of the bracket.
|
||
|
||
We have indicated in Fig. 1.2(a) that the bracket is fastened to a very thick steel column. The description “very thick” is of course relative to the thickness t and the height h of the bracket. We translate this statement into the assumption that the bracket is fastened to a (practically) rigid column. Hence we can focus our attention on the bracket by applying a “rigid column boundary condition” to it. (Of course, at a later time, an analysis of the column may be required, and then the loads carried by the two bolts, as a consequence of the load W, will need to be applied to the column.)
|
||
|
||
We also assume that the load W is applied very slowly. The condition of time “very slowly” is relative to the largest natural period of the bracket; that is, the time span over which the load W is increased from zero to its full value is much longer than the fundamental period of the bracket. We translate this statement into requiring a static analysis (and not a dynamic analysis).
|
||
|
||
<!-- source-page: 22 -->
|
||
|
||
With these preliminary considerations we can now establish an appropriate mathematical model for the analysis of the bracket—depending on what phenomena are to be predicted. Let us assume, in the first instance, that only the total bending moment at section AA in the bracket and the deflection at the load application are sought. To predict these quantities, we consider a beam mathematical model including shear deformations [see Fig. 1.2(b)] and obtain
|
||
|
||
$$
|
||
\begin{array}{l} \begin{array}{r l} \boldsymbol {M} & = \boldsymbol {W L} \\ & = 2 7. 5 0 0 \mathrm{N} \end{array} \tag {1.1} \\ = 2 7, 5 0 0 \mathrm{N} \mathrm{cm} \\ \end{array}
|
||
$$
|
||
|
||
$$
|
||
\delta \left| _ {\text { at load } W} = \frac {1}{3} \frac {W (L + r _ {N}) ^ {3}}{E I} + \frac {W (L + r _ {N})}{\frac {5}{6} A G} \right. \tag {1.2}
|
||
$$
|
||
|
||
$$
|
||
= 0. 0 5 3 \mathrm{cm}
|
||
$$
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
Two bolts
|
||
Uniform thickness t
|
||
A
|
||
h
|
||
rN
|
||
A
|
||
L
|
||
W
|
||
Pin
|
||
W = 1000 N
|
||
L = 27.5 cm
|
||
rN = 0.5 cm
|
||
E = 2 × 10^7 N/cm^2
|
||
v = 0.3
|
||
h = 6.0 cm
|
||
t = 0.4 cm
|
||
Very thick steel column
|
||
</details>
|
||
|
||
(a) Physical problem of steel bracket
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
A
|
||
rN = 0.5 cm
|
||
W = 1000 N
|
||
h = 6 cm
|
||
x
|
||
δ
|
||
L + rN = 28 cm
|
||
A
|
||
</details>
|
||
|
||
(b) Beam model
|
||
Figure 1.2 Bracket to be analyzed and two mathematical models
|
||
|
||
<!-- source-page: 23 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
Areas with imposed zero displacements u, v
|
||
τnn
|
||
τnt
|
||
n
|
||
t
|
||
y, v
|
||
z, w
|
||
x, u
|
||
Hole
|
||
B
|
||
W
|
||
Load applied at point B
|
||
</details>
|
||
|
||
Equilibrium equations (see Example 4.2)
|
||
|
||
$$
|
||
\left. \begin{array}{l} \frac {\partial \tau_ {x x}}{\partial x} + \frac {\partial \tau_ {x y}}{\partial y} = 0 \\ \frac {\partial \tau_ {y x}}{\partial x} + \frac {\partial \tau_ {y y}}{\partial y} = 0 \end{array} \right\} \text {in domain of bracket}
|
||
$$
|
||
|
||
$$
|
||
\begin{array}{r l} \tau_ {n n} & = 0, \tau_ {n t} = 0 \text { on surfaces except at point } B \\ & \text { and at imposed zero displacements } \end{array}
|
||
$$
|
||
|
||
Stress-strain relation (see Table 4.3):
|
||
|
||
$$
|
||
\left[ \begin{array}{l} \tau_ {x x} \\ \tau_ {y y} \\ \tau_ {x y} \end{array} \right] = \frac {E}{1 - \nu^ {2}} \left[ \begin{array}{c c c} 1 & \nu & 0 \\ \nu & 1 & 0 \\ 0 & 0 & (1 - \nu) / 2 \end{array} \right] \left[ \begin{array}{l} \epsilon_ {x x} \\ \epsilon_ {y y} \\ \gamma_ {x y} \end{array} \right]
|
||
$$
|
||
|
||
$$
|
||
E = \text { Young's modulus }, \nu = \text { Poisson's ratio }
|
||
$$
|
||
|
||
Strain-displacement relations (see Section 4.2):
|
||
|
||
$$
|
||
\epsilon_ {x x} = \frac {\partial u}{\partial x}; \quad \epsilon_ {y y} = \frac {\partial v}{\partial y}; \quad \gamma_ {x y} = \frac {\partial u}{\partial y} + \frac {\partial v}{\partial x}
|
||
$$
|
||
|
||
(c) Plane stress model
|
||
|
||
Figure 1.2 (continued)
|
||
|
||
where $L$ and $r_N$ are given in Fig. 1.2(a), $E$ is the Young's modulus of the steel used, $G$ is the shear modulus, $I$ is the moment of inertia of the bracket arm ( $I = \frac{1}{12} h^3 t$ ), $A$ is the cross-sectional area ( $A = ht$ ), and the factor $\frac{5}{6}$ is a shear correction factor (see Section 5.4.1).
|
||
|
||
Of course, the relations in (1.1) and (1.2) assume linear elastic infinitesimal displacement conditions, and hence the load must not be so large as to cause yielding of the material and/or large displacements.
|
||
|
||
Let us now ask whether the mathematical model used in Fig. 1.2(b) was reliable and effective. To answer this question, strictly, we should consider a very-comprehensive mathematical model, which in this case would be a fully three-dimensional representation of the
|
||
|
||
<!-- source-page: 24 -->
|
||
|
||
full bracket. This model should include the two bolts fastening the bracket to the (assumed rigid) column as well as the pin through which the load W is applied. The three-dimensional solution of this model using the appropriate geometry and material data would give the numbers against which we would compare the answers given in (1.1) and (1.2). Note that this three-dimensional mathematical model contains contact conditions (the contact is between the bolts, the bracket, and the column, and between the pin carrying the load and the bracket) and stress concentrations in the fillets and at the holes. Also, if the stresses are high, nonlinear material conditions should be included in the model. Of course, an analytical solution of this mathematical model is not available, and all we can obtain is a numerical solution. We describe in this book how such solutions can be calculated using finite element procedures, but we may note here already that the solution would be relatively expensive in terms of computer resources and engineering time used.
|
||
|
||
Since the three-dimensional comprehensive mathematical model is very likely too comprehensive a model (for the analysis questions we have posed), we instead may consider a linear elastic two-dimensional plane stress model as shown in Fig. 1.2(c). This mathematical model represents the geometry of the bracket more accurately than the beam model and assumes a two-dimensional stress situation in the bracket (see Section 4.2). The bending moment at section AA and deflection under the load calculated with this model can be expected to be quite close to those calculated with the very-comprehensive three-dimensional model, and certainly this two-dimensional model represents a higher-order model against which we can measure the adequacy of the results given in (1.1) and (1.2). Of course, an analytical solution of the model is not available, and a numerical solution must be sought.
|
||
|
||
Figures 1.3(a) to (e) show the geometry and the finite element discretization used in the solution of the plane stress mathematical model and some stress and displacement results obtained with this discretization. Let us note the various assumptions of this mathematical model when compared to the more comprehensive three-dimensional model discussed earlier. Since a plane stress condition is assumed, the only nonzero stresses are $\tau_{xx}$ , $\tau_{yy}$ , and $\tau_{xy}$ . Hence we assume that the stresses $\tau_{zz}$ , $\tau_{yz}$ , and $\tau_{zx}$ are zero. Also, the actual bolt fastening and contact conditions between the steel column and the bracket are not included.
|
||
|
||
|
||
|
||
<details>
|
||
<summary>natural_image</summary>
|
||
|
||
Simple line drawing of a T-shaped mechanical or electrical component with four circular holes (no text or symbols)
|
||
</details>
|
||
|
||
(a) Geometry of bracket as obtained from a CAD program
|
||
Figure 1.3 Plane stress analysis of bracket in Fig. 1.2. AutoCAD was used to create the geometry, and ADINA was used for the finite element analysis.
|
||
|
||
<!-- source-page: 25 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>natural_image</summary>
|
||
|
||
Pure technical diagram of a mechanical linkage or beam with symmetrical supports and meshed sections (no text or symbols)
|
||
</details>
|
||
|
||
(b) Mesh of nine-node elements used in finite element discretization
|
||
|
||
|
||
|
||
<details>
|
||
<summary>natural_image</summary>
|
||
|
||
Diagram of a vehicle with two wheels and a connecting rod, showing structural grid and flow lines (no text or labels)
|
||
</details>
|
||
|
||
(c) Deflected shape. Deflections are drawn with a magnification factor of 100 together with the original configuration
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
00000000
|
||
TIME: 1:000
|
||
17000
|
||
12000
|
||
7000
|
||
000
|
||
</details>
|
||
|
||
(d) Maximum principal stress near notch. Unsmoothed stress results are shown. The small breaks in the bands indicate that a reasonably accurate solution of the mathematical model has been obtained (see Section 4.3.6)
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
SINHITANEO
|
||
SINHITANEO
|
||
TIME: 1000
|
||
-700
|
||
-1000
|
||
-1500
|
||
-2000
|
||
</details>
|
||
|
||
(e) Maximum principal stress near notch. Smoothed stress results. (The averages of nodal point stresses are taken and interpolated over the elements.)
|
||
Figure 1.3 (continued)
|
||
|
||
<!-- source-page: 26 -->
|
||
|
||
in the model, and the pin carrying the load into the bracket is not modeled. However, since our objective is only to predict the bending moment at section AA and the deflection at point B, these assumptions are deemed reasonable and of relatively little influence.
|
||
|
||
Let us assume that the results obtained in the finite element solution of the mathematical model are sufficiently accurate that we can refer to the solution given in Fig. 1.3. as the solution of the plane stress mathematical model.
|
||
|
||
Figure 1.3(c) shows the calculated deformed configuration. The deflection at the point of load application B as predicted in the plane stress solution is
|
||
|
||
$$
|
||
\delta \left| _ {\text { at load } w} = 0. 0 6 4 \mathrm{cm} \right. \tag {1.3}
|
||
$$
|
||
|
||
Also, the total bending moment predicted at section AA is
|
||
|
||
$$
|
||
M | _ {x = 0} = 2 7, 5 0 0 \mathrm{N} \mathrm{cm} \tag {1.4}
|
||
$$
|
||
|
||
Whereas the same magnitude of bending moment at section AA is predicted by the beam model and the plane stress model, $^{1}$ the deflection of the beam model is considerably less than that predicted by the plane stress model [because of the assumption that the beam in Fig. 1.2(b) is supported rigidly at its left end, which neglects any deformation between the beam end and the bolts].
|
||
|
||
Considering these results, we can say that the beam mathematical model in Fig. 1.2(b) is reliable if the required bending moment is to be predicted within 1 percent and the deflection is to be predicted only within 20 percent accuracy. The beam model is of course also effective because the calculations are performed with very little effort.
|
||
|
||
On the other hand, if we next ask for the maximum stress in the bracket, then the simple mathematical beam model in Fig. 1.2(b) will not yield a sufficiently accurate answer. Specifically, the beam model totally neglects the stress increase due to the fillets. $^{2}$ Hence a plane stress solution including the fillets is necessary.
|
||
|
||
The important points to note here are the following.
|
||
|
||
1. The selection of the mathematical model must depend on the response to be predicted (i.e., on the questions asked of nature).
|
||
2. The most effective mathematical model is that one which delivers the answers to the questions in a reliable manner (i.e., within an acceptable error) with the least amount of effort.
|
||
3. A finite element solution can solve accurately only the chosen mathematical model (e.g., the beam model or the plane stress model in Fig. 1.2) and cannot predict any more information than that contained in the model.
|
||
4. The notion of reliability of the mathematical model hinges upon an accuracy assessment of the results obtained with the chosen mathematical model (in response to the questions asked) against the results obtained with the very-comprehensive mathematical model. However, in practice the very-comprehensive mathematical model is
|
||
|
||
$^{1}$ The bending moment at section AA in the plane stress model is calculated here from the finite element nodal point forces, and for this statically determinate analysis problem the internal resisting moment must be equal to the externally applied moment (see Example 4.9).
|
||
|
||
$^{2}$ Of course, the effect of the fillets could be estimated by the use of stress concentration factors that have been established from plane stress solutions.
|
||
|
||
<!-- source-page: 27 -->
|
||
|
||
usually not solved, and instead engineering experience is used, or a more refined mathematical model is solved, to judge whether the mathematical model used was adequate (i.e., reliable) for the response to be predicted.
|
||
|
||
Finally, there is one further important general point. The chosen mathematical model may contain extremely high stresses because of sharp corners, concentrated loads, or other effects. These high stresses may be due solely to the simplifications used in the model when compared with the very-comprehensive mathematical model (or with nature). For example, the concentrated load in the plane stress model in Fig. 1.2(c) is an idealization of a pressure load over a small area. (This pressure would in nature be transmitted by the pin carrying the load into the bracket.) The exact solution of the mathematical model in Fig. 1.2(c) gives an infinite stress at the point of load application, and we must therefore expect a very large stress at point B as the finite element mesh is refined. Of course, this very large stress is an artifice of the chosen model, and the concentrated load should be replaced by a pressure load over a small area when a very fine discretization is used (see further discussion). Furthermore, if the model then still predicts a very high stress, a nonlinear mathematical model would be appropriate.
|
||
|
||
Note that the concentrated load in the beam model in Fig. 1.2(b) does not introduce any solution difficulties. Also, the right-angled sharp corners at the support of the beam model, of course, do not introduce any solution difficulties, whereas such corners in a plane stress model would introduce infinite stresses. Hence, for the plane stress model, the corners have to be rounded to more accurately represent the geometry of the actual physical bracket.
|
||
|
||
We thus realize that the solution of a mathematical model may result in artificial difficulties that are easily removed by an appropriate change in the mathematical model to more closely represent the actual physical situation. Furthermore, the choice of a more encompassing mathematical model may result, in such cases, in a decrease in the required solution effort.
|
||
|
||
While these observations are of a general nature, let us consider once again, specifically, the use of concentrated loads. This idealization of load application is extensively used in engineering practice. We now realize that in many mathematical models (and therefore also in the finite element solutions of these models), such loads create stresses of infinite value. Hence, we may ask under what conditions in engineering practice solution difficulties may arise. We find that in practice solution difficulties usually arise only when the finite element discretization is very fine, and for this reason the matter of infinite stresses under concentrated loads is frequently ignored. As an example, Fig. 1.4 gives finite element results obtained in the analysis of a cantilever, modeled as a plane stress problem. The cantilever is subjected to a concentrated tip load. In practice, the $6 \times 1$ mesh is usually considered sufficiently fine, and clearly, a much finer discretization would have to be used to accurately show the effects of the stress singularities at the point of load application and at the support. As already pointed out, if such a solution is pursued, it is necessary to change the mathematical model to more accurately represent the actual physical situation of the structure. This change in the mathematical model may be important in self-adaptive finite element analyses because in such analyses new meshes are generated automatically and artificial stress singularities cause—artificially—extremely fine discretizations.
|
||
|
||
We refer to these considerations in Section 4.3.4 when we state the general elasticity problem considered for finite element solution.
|
||
|
||
<!-- source-page: 28 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
20
|
||
W = 0.1
|
||
E = 200,000
|
||
v = 0.30
|
||
Thickness = 0.1
|
||
δ
|
||
1.0
|
||
</details>
|
||
|
||
(a) Geometry, boundary conditions, and material data. Bernoulli beam theory results: $\delta = 0.16$ , $\tau_{max} = 120$
|
||
|
||
|
||
|
||
<details>
|
||
<summary>text_image</summary>
|
||
|
||
w
|
||
y
|
||
x
|
||
</details>
|
||
|
||
(b) Typical finite element discretization, $6 \times 1$ mesh of 9-node elements; results are: $\delta = 0.16$ , $\tau_{max} = 116$
|
||
Figure 1.4 Analysis of a cantilever as a plane stress problem
|
||
|
||
In summary, we should keep firmly in mind that the crucial step in any finite element analysis is always choosing an appropriate mathematical model since a finite element solution solves only this model. Furthermore, the mathematical model must depend on the analysis questions asked and should be reliable and effective (as defined earlier). In the process of analysis, the engineer has to judge whether the chosen mathematical model has been solved to a sufficient accuracy and whether the chosen mathematical model was appropriate (i.e., reliable) for the questions asked. Choosing the mathematical model, solving the model by appropriate finite element procedures, and judging the results are the fundamental ingredients of an engineering analysis using finite element methods.
|
||
|
||
# 1.3 FINITE ELEMENT ANALYSIS AS AN INTEGRAL PART OF COMPUTER-AIDED ENGINEERING
|
||
|
||
Although a most exciting field of activity, engineering analysis is clearly only a support activity in the larger field of engineering design. The analysis process helps to identify good new designs and can be used to improve a design with respect to performance and cost.
|
||
|
||
In the early use of finite element methods, only specific structures were analyzed, mainly in the aerospace and civil engineering industries. However, once the full potential of finite element methods was realized and the use of computers increased in engineering design environments, emphasis in research and development was placed upon making the use of finite element methods an integral part of the design process in mechanical, civil, and aeronautical engineering.
|
||
|
||
<!-- source-page: 29 -->
|
||
|
||
|
||
|
||
<details>
|
||
<summary>flowchart</summary>
|
||
|
||
```mermaid
|
||
graph TD
|
||
A["Interactive use of software"] --> B["Automatic drafting"]
|
||
B --> C["Data base"]
|
||
C --> D["Geometry generation"]
|
||
D --> E["Finite element analysis"]
|
||
E --> F["Kinematic analysis"]
|
||
F --> G["Cam"]
|
||
G --> H["Numerical control"]
|
||
H --> I["Robotics"]
|
||
I --> J["Assemblage process"]
|
||
J --> K["Management of process"]
|
||
K --> L["Automatized workshop"]
|
||
C --> M["CAD"]
|
||
C --> N["CAM"]
|
||
```
|
||
</details>
|
||
|
||
Figure 1.5 The field of CAE viewed schematically
|
||
|
||
Figure 1.5 gives a schematic of the steps in computer-aided engineering, see K. J. Bathe [C, D, H]. Finite element analysis is only a part of the complete process, but it is an important part.
|
||
|
||
We note that the first step in Figure 1.5 is the creation of a geometric representation of the design part. Many different computer programs can be employed (e.g., a typical and popular program is AutoCAD). In this step, the material properties, the applied loading and boundary conditions on the geometry also need to be defined. Given this information, a finite element analysis may proceed. Since the geometry and other data of the actual physical part may be quite complex, it is usually necessary to simplify the geometry and loading in order to reach a tractable mathematical model. Of course, the mathematical model should be reliable and effective for the analysis questions posed, as discussed in the preceding section. The finite element analysis solves the chosen mathematical model, which may be changed and evolve depending on the purpose of the analysis (see Fig. 1.1).
|
||
|
||
Considering this process—which generally is and should be performed by engineering designers and not only specialists in analysis—we recognize that the finite element methods must be very reliable and robust. By reliability of the finite element methods we now $^{3}$ mean that in the solution of a well-posed mathematical model, the finite element procedures should always for a reasonable finite element mesh give a reasonable solution,
|
||
|
||
<!-- source-page: 30 -->
|
||
|
||
and if the mesh is reasonably fine, an accurate solution should always be obtained. By robustness of the finite element methods we mean that the performance of the finite element procedures should not be unduly sensitive to the material data, the boundary conditions, and the loading conditions used. Therefore, finite element procedures that are not robust will also not be reliable.
|
||
|
||
For example, assume that in the plane stress solution of the mathematical model in Fig. 1.2(c), any reasonable finite element discretization using a certain element type is employed. Then the solution obtained from any such analysis should not be hugely in error, that is, an order of magnitude larger (or smaller) than the exact solution. Using an unreliable finite element for the discretization would typically lead to good solutions for some mesh topologies, whereas with other mesh topologies it would lead to bad solutions. Elements based on reduced integration with spurious zero energy modes can show this unreliable behavior (see Section 5.5.6).
|
||
|
||
Similarly, assume that a certain finite element discretization of a mathematical model gives accurate results for one set of material parameters and that a small change in the parameters corresponds to a small change in the exact solution of the mathematical model. Then the same finite element discretization should also give accurate results for the mathematical model with the small change in material parameters and not yield results that are very much in error.
|
||
|
||
These considerations regarding effective finite element discretizations are very important and are discussed in the presentation of finite element discretizations and their stability and convergence properties (see Chapters 4 to 7). For use in engineering design, it is of utmost importance that the finite element methods be reliable, robust, and of course efficient. Reliability and robustness are important because a designer has relatively little time for the process of analysis and must be able to obtain an accurate solution of the chosen mathematical model quickly and without “trial and error.” The use of unreliable finite element methods is simply unacceptable in engineering practice.
|
||
|
||
A general aim in a finite element analysis is also the calculation of error estimates, that is, estimates of how closely the finite element solution approximates the exact solution of the solution of the mathematical model (see Section 4.3.6). These estimates indicate whether a specific finite element discretization has indeed yielded an accurate response prediction, and a designer can then rationally decide whether the given results should be used. In the case that unacceptable results have been obtained, perhaps by using unreliable finite element methods, the difficulty is of course how to obtain accurate results.
|
||
|
||
Finally, we venture to comment on the future of finite element methods in CAE and the engineering sciences. Surely, many designers do not have time to study finite element methods in depth. Their sole objective is to use these techniques to enhance the design product. Hence the integrated use of finite element methods in CAE ideally involves less scrutiny of finite element meshes during the analysis, so that the engineer can focus on the actual questions related to the design. This has now been achieved to some extent, but a fully automatic solution involving all steps of analysis is so far only possible some simple design questions. The aspects of human judgments and solution costs play major roles in complex analyses involving dynamic or nonlinear response solutions, including the selection of an appropriate mathematical model, see M.L. Bucalem and K.J. Bathe [B], and may require considerable analysis expertise. Also, the simulations sought become increasingly more complex, involving not only solids and structures, but multiphysics phenomena with solids, fluids, piezoelectrics, electromagnetics and their interactions, see for example K. J. Bathe [I, K, L], P. Gaudenzi and K. J. Bathe [A], K. J. Bathe, H. Zhang, and Y. Yan [A] and C. Deilmann and K. J. Bathe [A].
|