The following four-article series was published recently
in a Newsletter of the American Society of Mechanical
Engineers (ASME). It serves as an introduction to the
recent analysis discipline known as the Finite Element
Method. The author is an engineering consultant special-
izing in Finite Element Analysis, and may be reached at:
Roensch Engineering Consulting
634 Lake Shore Road
Grafton, WI 53024-9723
414-375-2228
---------------------------
First in a four-part series
---------------------------
Finite element analysis (FEA) is a fairly recent discipline crossing the
boundaries of mathematics, physics, engineering and computer science. The
method has wide application and enjoys extensive utilization in the
structural, thermal and fluid analysis areas. The finite element method is
comprised of three major phases: (1) pre-processing, in which the analyst
develops a finite element mesh to divide the subject geometry into
subdomains for mathematical analysis, and applies material properties and
boundary conditions, (2) solution, during which the program derives the
governing matrix equations from the model and solves for the primary
quantities, and (3) post-processing, in which the analyst checks the
validity of the solution, examines the values of primary quantities (such
as displacements and stresses), and derives and examines additional
quantities (such as specialized stresses and error indicators).
The advantages of FEA are numerous and important. A new design concept may
be modeled to determine its real world behavior under various load
environments, and may therefore be refined prior to the creation of
drawings, when few dollars have been committed and changes are inexpensive.
Once a detailed CAD model has been developed, FEA can analyze the design in
detail, saving time and money by reducing the number of prototypes
required. An existing product which is experiencing a field problem, or is
simply being improved, can be analyzed to speed an engineering change and
reduce its cost. In addition, FEA can be performed on increasingly
affordable computer workstations, and professional assistance is available.
It is also important to recognize the limitations of FEA. Commercial
software packages and the required hardware, while coming down in price,
still require a significant investment. The method can reduce product
testing, but cannot totally replace it. Probably most important, an
inexperienced user can deliver incorrect answers, upon which expensive
decisions will be based. FEA is a demanding tool, in that the analyst must
be proficient not only in elasticity or fluids, but also in mathematics,
computer science, and especially the finite element method itself.
Which FEA package to use is a subject that cannot possibly be covered in
this short discussion, and the choice involves personal preferences as well
as package functionality. Where to run the package, on the other hand, is
becoming increasingly clear. A typical finite element solution creates a
temporary matrix file as large as 1 Gbyte, with 50 to 100 Mbytes common,
thus requiring a fast, modern disk subsystem for acceptable performance.
Memory requirements are of course dependent on the code, but in the
interest of performance, the more the better, with 8 to 32 Mbytes per user
a representative range. Processing power is the final link in the
performance chain, with clock speed, cache, pipelining and vector
processing all contributing to the bottom line. All in all, today's user
needs a minimum of 1 or 2 Mflops (millions of double-precision
floating-point operations per second) sustained performance, with 10 or 20
Mflops being all the better. These analyses can run for hours or even days
on the fastest systems, so computing power is of the essence. Given these
requirements, performing FEA on a PC may be suitable for teaching the
method, but is likely to be found insufficient for dedicated analysis.
Until very recently, only an expensive host could fulfill the needs of a
full-time analyst. (Unfortunately, unleashing several solutions without
careful priority control could all but kill the interactive productivity of
time-shared users.) Today, however, powerful engineering workstations
provide an affordable platform for FEA, and are rapidly becoming the system
of choice. Expect to pay $50K to $200K for station and software, depending
on hardware performance and software capability.
One aspect often overlooked when entering the finite element area is
education. Without adequate training on the finite element method and the
specific FEA package, a new user will not be productive in a reasonable
amount of time, and may in fact fail miserably. Expect to dedicate one to
two weeks up front, and another one to two weeks over the first year, to
either classroom or self-help education. It is also important that the
user have a basic understanding of the computer's operating system.
Next month's article will go into detail on the pre-processing phase of the
finite element method.
--------------------------------------------------------------------------
Steve Roensch is an engineering consultant specializing in finite element
analysis. (C) 1991 Roensch Engineering Consulting, 414-375-2228
--------------------------------------------------------------------------
----------------------------
Second in a four-part series
----------------------------
As discussed last month, finite element analysis is comprised of
pre-processing, solution and post-processing phases. The goals of
pre-processing are to develop an appropriate finite element mesh, assign
suitable material properties, and apply boundary conditions in the form of
restraints and loads.
The finite element mesh subdivides the geometry into elements, upon which
are found nodes. The nodes, which are really just point locations in
space, are generally located at the element corners and perhaps near each
midside. For a two-dimensional (2D) analysis, or a three-dimensional (3D)
thin shell analysis, the elements are essentially 2D, but may be "warped"
slightly to conform to a 3D surface. An example is the thin shell linear
quadrilateral; thin shell implies essentially classical shell theory,
linear defines the interpolation of mathematical quantities across the
element, and quadrilateral describes the geometry. For a 3D solid
analysis, the elements have physical thickness in all three dimensions.
Common examples include solid linear brick and solid parabolic tetrahedral
elements. In addition, there are many special elements, such as
axisymmetric elements for situations in which the geometry, material and
boundary conditions are all symmetric about an axis.
The model's degrees of freedom (dof) are assigned at the nodes. Solid
elements generally have three translational dof per node. Rotations are
accomplished through translations of groups of nodes relative to other
nodes. Thin shell elements, on the other hand, have six dof per node:
three translations and three rotations. The addition of rotational dof
allows for evaluation of quantities through the shell, such as bending
stresses due to rotation of one node relative to another. Thus, for
structures in which classical thin shell theory is a valid approximation,
carrying extra dof at each node bypasses the necessity of modeling the
physical thickness. The assignment of nodal dof also depends on the class
of analysis. For a thermal analysis, for example, only one temperature dof
exists at each node.
Developing the mesh is usually the most time-consuming task in FEA. In the
past, node locations were keyed in manually to approximate the geometry.
The more modern approach is to develop the mesh directly on the CAD
geometry, which will be (1) wireframe, with points and curves representing
edges, (2) surfaced, with surfaces defining boundaries, or (3) solid,
defining where the material is. Solid geometry is preferred, but often a
surfacing package can create a complex blend that a solids package will not
handle. As far as geometric detail, an underlying rule of FEA is to "model
what is there", and yet simplifying assumptions simply must be applied to
avoid huge models. Analyst experience is of the essence.
The geometry is meshed with a mapping algorithm or an automatic
free-meshing algorithm. The first maps a rectangular grid onto a geometric
region, which must therefore have the correct number of sides. Mapped
meshes can use the accurate and cheap solid linear brick 3D element, but
can be very time-consuming, if not impossible, to apply to complex
geometries. Free-meshing automatically subdivides meshing regions into
elements, with the advantages of fast meshing, easy mesh-size transitioning
(for a denser mesh in regions of large gradient), and adaptive
capabilities. Disadvantages include generation of huge models, generation
of distorted elements, and, in 3D, the use of the rather expensive solid
parabolic tetrahedral element. It is always important to check elemental
distortion prior to solution. A badly distorted element will cause a
matrix singularity, killing the solution. A less distorted element may
solve, but can deliver very poor answers. Acceptable levels of distortion
are dependent upon the solver being used.
Material properties required vary with the type of solution. A linear
statics analysis, for example, will require an elastic modulus, Poisson's
ratio and perhaps a density for each material. Examples of restraints are
declaring a nodal translation or temperature. Loads include forces,
pressures and heat flux. It is preferable to apply boundary conditions to
the CAD geometry, with the FEA package transferring them to the underlying
model, to allow for simpler application of adaptive and optimization
algorithms. It is worth noting that the largest error in the entire
process is often in the boundary conditions. Running multiple cases as a
sensitivity analysis may be required.
Next month's article will discuss the solution phase of the finite element
method.
--------------------------------------------------------------------------
Steve Roensch is an engineering consultant specializing in finite element
analysis. (C) 1991 Roensch Engineering Consulting, 414-375-2228
--------------------------------------------------------------------------
---------------------------
Third in a four-part series
---------------------------
While the pre-processing and post-processing phases of the finite element
method are interactive and time-consuming for the analyst, the solution is
usually a batch process, and is demanding of computer resource. The
governing equations are assembled into matrix form and are solved
numerically. The assembly process depends not only on the type of analysis
(e.g. static or dynamic), but also on the model's element types and
properties, material properties and boundary conditions.
In the case of a linear static structural analysis, the assembled equation
is of the form Kd = r, where K is the system stiffness matrix, d is the
nodal degree of freedom (dof) displacement vector, and r is the applied
nodal load vector. To appreciate this equation, one must begin with the
underlying elasticity theory. The strain-displacement relation may be
introduced into the stress-strain relation to express stress in terms of
displacement. Under the assumption of compatibility, the differential
equations of equilibrium in concert with the boundary conditions then
determine a unique displacement field solution, which in turn determines
the strain and stress fields. The chances of directly solving these
equations are slim to none for anything but the most trivial geometries,
hence the need for approximate numerical techniques presents itself.
A finite element mesh is actually a displacement-nodal displacement
relation, which, through the element interpolation scheme, determines the
displacement anywhere in an element given the values of its nodal dof.
Introducing this relation into the strain-displacement relation, we may
express strain in terms of the nodal displacement, element interpolation
scheme and differential operator matrix. Recalling that the expression for
the potential energy of an elastic body includes an integral for strain
energy stored (dependent upon the strain field) and integrals for work done
by external forces (dependent upon the displacement field), we can
therefore express system potential energy in terms of nodal displacement.
Applying the principle of minimum potential energy, we may set the partial
derivative of potential energy with respect to the nodal dof vector to
zero, resulting in: a summation of element stiffness integrals, multiplied
by the nodal displacement vector, equals a summation of load integrals.
Each stiffness integral results in an element stiffness matrix, which sum
to produce the system stiffness matrix, and the summation of load integrals
yields the applied load vector, resulting in Kd = r. In practice,
integration rules are applied to elements, loads appear in the r vector,
and nodal dof boundary conditions may appear in the d vector or may be
partitioned out of the equation.
Solution methods for finite element matrix equations are plentiful. In the
case of the linear static Kd = r, inverting K is computationally expensive
and numerically unstable. A better technique is Cholesky factorization, a
form of Gauss elimination, and a minor variation on the the "LDU"
factorization theme. The K matrix may be efficiently factorized into LDU,
where L is lower triangular, D is diagonal, and U is upper triangular,
resulting in LDUd = r. Since L and D are easily inverted, and U is upper
triangular, d may be determined by back-substitution. Another popular
approach is the wavefront method, which assembles and reduces the equations
at the same time. The key point is that the analyst must understand the
solution technique being applied.
Dynamic analysis for too many analysts means normal modes. Knowledge of
the natural frequencies and mode shapes of a design may be enough in the
case of a single-frequency vibration of an existing product or prototype,
with FEA being used to investigate the effects of mass, stiffness and
damping modifications. When investigating a future product, or an existing
design with multiple modes excited, forced response modeling should be used
to apply the expected transient or frequency environment to estimate the
displacement and even dynamic stress at each time step.
This discussion has assumed h-code elements, for which the order of the
interpolation polynomials is fixed. Another technique, p-code, increases
the order iteratively until convergence, with error estimates available
after one analysis. Finally, the boundary element method places elements
only along the geometrical boundary. These techniques have limitations,
but expect to see more of them in the near future.
Next month's article will discuss the post-processing phase of the finite
element method.
--------------------------------------------------------------------------
Steve Roensch is an engineering consultant specializing in finite element
analysis. (C) 1991 Roensch Engineering Consulting, 414-375-2228
--------------------------------------------------------------------------
--------------------------
Last in a four-part series
--------------------------
After a finite element model has been prepared and checked, boundary
conditions have been applied, and the model has been solved, it is time to
investigate the results of the analysis. This activity is known as the
post-processing phase of the finite element method.
Post-processing begins with a thorough check for problems that may have
occurred during solution. Most solvers provide a log file, which should be
searched for warnings or errors, and which will also provide a quantitative
measure of how well-behaved the numerical procedures were during solution.
Next, reaction loads at restrained nodes should be summed and examined as a
"sanity check". Reaction loads that do not closely balance the applied
load resultant for a linear static analysis should cast doubt on the
validity of other results. Error norms such as strain energy density and
stress deviation among adjacent elements might be looked at next, but for
h-code analyses these quantities are best used to target subsequent
adaptive remeshing.
Once the solution is verified to be free of numerical problems, the
quantities of interest may be examined. Many display options are
available, the choice of which depends on the mathematical form of the
quantity as well as its physical meaning. For example, the displacement of
a solid linear brick element's node is a 3-component spatial vector, and
the model's overall displacement is often displayed by superposing the
deformed shape over the undeformed shape. Dynamic viewing and animation
capabilities aid greatly in obtaining an understanding of the deformation
pattern. Stresses, being tensor quantities, currently lack a good single
visualization technique, and thus derived stress quantities are extracted
and displayed. Principle stress vectors may be displayed as color-coded
arrows, indicating both direction and magnitude. The magnitude of
principle stresses or of a scalar failure stress such as the Von Mises
stress may be displayed on the model as colored bands. When this type of
display is treated as a 3D object subjected to light sources, the resulting
image is known as a shaded image stress plot. Displacement magnitude may
also be displayed by colored bands, but this can lead to misinterpretation
as a stress plot.
An area of post-processing that is rapidly gaining popularity is that of
adaptive remeshing. Error norms such as strain energy density are used to
remesh the model, placing a denser mesh in regions needing improvement and
a coarser mesh in areas of overkill. Adaptivity requires an associative
link between the model and the underlying CAD geometry, and works best if
boundary conditions may be applied directly to the geometry, as well.
Adaptive remeshing is a recent demonstration of the iterative nature of
h-code analysis.
Optimization is another area enjoying recent advancement. Based on the
values of various results, the model is modified automatically in an
attempt to satisfy certain performance criteria and is solved again. The
process iterates until some convergence criterion is met. In its scalar
form, optimization modifies beam cross-sectional properties, thin shell
thicknesses and/or material properties in an attempt to meet maximum stress
constraints, maximum deflection constraints, and/or vibrational frequency
constraints. Shape optimization is more complex, with the actual 3D model
boundaries being modified.
Another direction clearly visible in the finite element field is the
integration of FEA packages with so-called "mechanism" packages, which
analyze motion and forces of large-displacement multi-body systems. A
long-term goal would be real-time computation and display of displacements
and stresses in a multi-body system undergoing large displacement motion,
with frictional effects and fluid flow taken into account when necessary.
It is difficult to estimate the increase in computing power necessary to
accomplish this feat, but 2 or 3 orders of magnitude is probably close.
Algorithms to integrate these fields of analysis may be expected to follow
the computing power increases.
In summary, the finite element method is a relatively recent discipline
that has quickly become a mature method, especially for structural and
thermal analysis. The costs of applying this technology to everyday design
tasks have been dropping, while the capabilities delivered by the method
expand constantly. With education in the technique and in the commercial
software packages becoming more and more available, the question has moved
from "Why apply FEA?" to "Why not?". The method is fully capable of
delivering higher quality products in a shorter design cycle with a reduced
chance of field failure, provided it is applied by a capable analyst. It
is also a valid indication of thorough design practices, should an
unexpected litigation crop up. The time is now for industry to make
greater use of this and other analysis techniques.
--------------------------------------------------------------------------
Steve Roensch is an engineering consultant specializing in finite element
analysis. (C) 1991 Roensch Engineering Consulting, 414-375-2228
--------------------------------------------------------------------------
