 |
|||||||||||||||||||||||||
|
|||||||||||||||||||||||||
|
Chapter 7
Introduction to Finite Element Analysis in Solid Mechanics
Most practical design calculations involve components with a complicated three-dimensional geometry, and may also need to account for inherently nonlinear phenomena such as contact, large shape changes, or nonlinear material behavior.  These problems can only be solved using computer simulations. The finite element method is by far the most widely used and versatile technique for simulating deformable solids. This chapter gives a brief overview of the finite element method, with a view to providing the background needed to run simple simulations using a commercial finite element program. More advanced analysis requires a deeper understanding of the theory and implementation of finite element codes, which will be addressed in the next chapter.
HEALTH WARNING: It is deceptively easy to use commercial finite element software: most programs come with a nice user-interface that allows you to define the geometry of the solid, choose a material model, generate a finite element mesh and apply loads to the solid with a few mouse clicks.  If all goes well, the program will magically turn out animations showing the deformation; contours showing stress distributions; and much more besides. It is all too easy, however, to produce meaningless results, by attempting to solve a problem that does not have a well defined solution; by using an inappropriate numerical scheme; or simply using incorrect settings for internal tolerances in the code. In addition, even high quality software can contain bugs. Always treat the results of a finite element computations with skepticism!
7.1 A guide to using finite element software
The finite element method (FEM) is a computer technique for solving partial differential equations. One application is to predict the deformation and stress fields within solid bodies subjected to external forces. However, FEM can also be used to solve problems involving fluid flow, heat transfer, electromagnetic fields, diffusion, and many other phenomena.Â
The principle objective of the displacement based finite element method is to compute the displacement field within a solid subjected to external forces.
To make this precise, visualize a solid deforming under external loads. Every point in the solid moves as the load is applied. The displacement vector u(x) specifies the motion of the point at position x in the undeformed solid. Our objective is to determine u(x). Once u(x) is known, the strain and stress fields in the solid can be deduced.
There are two general types of finite element analysis in solid mechancis. In most cases, we are interested in determining the behavior of a solid body that is in static equilibrium. This means that both external and internal forces acting on the solid sum to zero. In some cases, we may be interested in the dynamic behavior of a solid body. Examples include modeling vibrations in structures, problems involving wave propagation, explosive loading and crash analysis.Â
For Dynamic
Problems the finite element method solves the equations of motion for a
continuum
For Static
Problems the finite element method solves the equilibrium equations
For some applications, you may also need to solve additional field equations. For example, you may be interested in calculating the temperature distribution in the solid, or calculating electric or magnetic fields. In addition, special finite element procedures are available to calculate buckling loads and their modes, as well as natural frequencies of vibration and the corresponding mode shapes for a deformable solid.Â
To set up a  finite element calculation, you will need to specify 1. The geometry of the solid. This is done by generating a finite element mesh for the solid. The mesh can usually be generated automatically from a CAD representation of the solid. 2. The properties of the material. This is done by specifying a constitutive law for the solid. 3. The nature of the loading applied to the solid. This is done by specifying the boundary conditions for the problem. 4.  If your analysis involves contact between two or more solids, you will need to specify the surfaces that are likely to come into contact, and the properties (e.g. friction coefficient) of the contact. 5. For a dynamic analysis, it is necessary to specify initial conditions for the problem. This is not necessary for a static analysis. 6. For problems involving additional fields, you may need to specify initial values for these field variables (e.g. you would need to specify the initial temperature distribution in a thermal analysis). You will also need to specify some additional aspects of the problem you are solving and the solution procedure to be used: 1. You will need to specify whether the computation should take into account finite changes in the geometry of the solid. 2. For a dynamic analysis, you will need to specify the time period of the analysis (or the number of time increments) 3. For a static analysis you will need to decide whether the problem is linear, or nonlinear.  Linear problems are very easy to solve. Nonlinear problems may need special procedures. 4. For a static analysis with history dependent materials you will need to specify the time period of the analysis, and the time step size (or number of steps) 5. If you are interested in calculating natural frequencies and mode shapes for the system, you must specify how many modes to extract.  6. Finally, you will need to specify what the finite element method must compute.
The steps in running a finite element computation are discussed in more detail in the following sections.
7.1.1 The Finite Element Mesh for a 2D or 3D component
The finite element mesh is used to specify the geometry of the solid, and is also used to describe the displacement field within the solid. A typical mesh (generated in the commercial FEA code ABAQUS) is shown in the picture to the right.
A finite element mesh may be three dimensional, like the example shown. Two dimensional finite element meshes are also used to model simpler modes of deformation. There are three main types of two dimensional finite element mesh: 1. Plane stress 2. Plane strain 3. Axisymmetric
In addition, special types of finite element can be used to model the overall behavior of a 3D solid, without needing to solve for the full 3D fields inside the solid. Examples are shell elements; plate elements; beam elements and truss elements. These will be discussed in a separate section below.
As before, only one quadrant of the specimen is meshed: symmetry boundary conditions will be enforced during the analysis.
The picture compares a three dimensional mesh of an axisymmetric bushing to an axisymmetric mesh. Note that the half the bushing has been cut away in the 3D view, to show the geometry more clearly. In an axisymmetric analysis, the origin for the (x,y) coordinate system is always on the axis of rotational symmetry. Note also that to run an axisymmetric finite element analysis, both the geometry of the solid, and also the loading applied to the solid, must have rotational symmetry about the y axis.
7.1.2 Nodes and Elements in a Mesh
A finite element mesh is defined by a set of nodes together with a set of finite elements, as shown in the sketch on the right.
1. A node
number. Every node is assigned an integer number,
which is used to identify the node.Â
Any convenient numbering scheme may be selected
2. Nodal
coordinates. For a three dimensional finite element
analysis, each node is assigned a set ofÂ
3. Nodal
displacements. Â When the solid deforms, each node moves to a
new position. For a three dimensional
finite element analysis, the nodal displacements specify the three components
of the displacement field u(x) at each node:
4. Other nodal degrees of freedom. For more complex analyses, we may wish to calculate a temperature distribution in the solid, or a voltage distribution, for example. In this case, each node is also assigned a temperature, voltage, or similar quantity of interest. There are also some finite element procedures which use more than just displacements to describe shape changes in a solid. For example, when analyzing two dimensional beams, we use the displacements and rotations of the beam at each nodal point to describe the deformation. In this case, each node has a rotation, as well as two displacement components. The collection of all unknown quantities (including displacements) at each node are known as degrees of freedom. A finite element program will compute values for these unknown degrees of freedom.
1. An element number. Every element is assigned an integer number, which is used to identify the element. Just as when numbering nodes, any convenient scheme may be selected to number elements.
2. A geometry. There are many possible shapes for an element. A few of the more common element types are shown in the picture. Nodes attached to the element are shown in red. In two dimensions, elements are generally either triangular or rectangular. In three dimensions, the elements are generally tetrahedra, hexahedra or bricks. There are other types of element that are used for special purposes: examples include truss elements (which are simply axial members), beam elements, and shell elements.Â
3. A set of faces. These are simply the sides of the element.
4. A set of nodes attached to the element. The picture on the right shows a typical finite element mesh. Element numbers are shown in blue, while node numbers are shown in red (some element and node numbers have been omitted for clarity).
All the elements are 8 noded quadrilaterals. Note that each element is connected to a set of nodes: element 1 has nodes (41, 45, 5, 1, 43, 25, 3, 21), element 2 has nodes (45, 49, 9, 5, 47, 29, 7, 25), and so on. It is conventional to list the nodes the nodes in the order given, with corner nodes first in order going counterclockwise around the element, followed by the midside nodes. The set of nodes attached to the element is known as the element connectivity.
5. An element
interpolation scheme. The purpose of a finite element is to
interpolate the displacement field u(x)
between values defined at the nodes.Â
This is best illustrated using an example. Consider the two dimensional, rectangular 4
noded element shown in the figure. Let
where
You can verify for yourself that the displacements have the correct values at the corners of the element, and the displacements evidently vary linearly with position within the element.
Different types of element interpolation scheme exist. The simple example described above is known as a linear element. Six noded triangles and 8 noded triangles are examples of quadratic elements: the displacement field varies quadratically with position within the element. In three dimensions, the 4 noded tetrahedron and the 8 noded brick are linear elements, while the 10 noded tet and 20 noded brick are quadratic.  Other special elements, such as beam elements or shell elements, use a more complex procedure to interpolate the displacement field.
Some special types of element interpolate both the
displacement field and some or all components of the stress field within an
element separately. (Usually, the displacement interpolation is sufficient to
determine the stress, since one can compute the strains at any point in the
element from the displacement, and then use the stress
6. Integration
points. One objective of a finite element analysis
is to determine the distribution of stress within a solid. This is done as follows. First, the displacements at each node are
computed (the technique used to do this will be discussed in Section 7.2 and
Chapter 8.)Â Then, the element interpolation
functions are used to determine the displacement at arbitrary points within
each element. The displacement field
can be differentiated to determine the strains. Once the strains are known, the stress
In principle, this procedure could be used to determine the stress at any point within an element. However, it turns out to work better at some points than others. The special points within an element where stresses are computed most accurately are known as integration points. (Stresses are sampled at these points in the finite element program to evaluate certain volume and area integrals, hence they are known as integration points).
For a detailed description of the locations of integration points within an element, you should consult an appropriate user manual. The approximate locations of integration points for a few two dimensional elements are shown in the figure.
There are some special types of element that use fewer integration points than those shown in the picture. These are known as reduced integration elements. This type of element is usually less accurate, but must be used to analyze deformation of incompressible materials (e.g. rubbers or rigid plastic metals).
7. A stress
7.1.3
Special Elements
If you need to analyze a solid with a special geometry (e.g. a simple truss, a structure made of one or more slender beams, or plates) it is not efficient to try to generate a full 3D finite element mesh for each member in the structure.  Instead, you can take advantage of the geometry to simplify the analysis.
The idea is quite simple. Instead of trying to calculate the full 3D displacement field in each member, the deformation is characterized by a reduced set of degrees of freedom. Specifically:
1. For a pin jointed truss, we simply calculate the displacement of each joint in the structure. The members are assumed to be in a state of uniaxial tension or compression, so the full displacement field within each member can be calculated in terms of joint displacements.
2. For a beam, we calculate the displacement and rotation of the cross section along the beam. These can be used to determine the internal shear forces bending moments, and therefore the stresses in the beam. A three dimensional beam has 3 displacement and 3 rotational degrees of freedom at each node.
3. For a plate, or shell, we again calculate the displacement and rotation of the
plate section. A three dimensional plate or shell has 3 displacement and two rotational degrees of freedom at
each node (these rotations characterize the rotation of a unit vector normal
to the plate). In some finite element
codes, nodes on plates and shells have a fictitious third rotational degree
of freedom which is added for convenience
In an analysis using truss, beam or plate elements, some additional information must be specified to set up the problem: 1. For a truss analysis, each member in the truss is a single element. The area of the member’s cross section must be specified. 2. For a beam analysis, the shape and orientation of the cross section must be specified (or, for an elastic analysis, you could specify the area moments of inertia directly).  There are also several versions of beam theory, which account differently for shape changes within the beam. Euler-Bernoulli beam theory is the simple version covered in introductory courses. Timoshenko beam theory is a more complex version, which is better for thicker beams. 3. For plates and shells, the thickness of the plate
must be given. In addition, the
deformation of the plate can be approximated in various ways
Calculations using beam and plate theory also differ from full 3D or 2D calculations in that both the deflection and rotation of the beam or plate must be calculated. This means that: 1. Nodes on beam elements have 6 degrees of freedom  2. Boundary conditions may constrain both displacement and rotational degrees of freedom. For example, to model a fully clamped boundary condition at the end of a beam (or the edge of a plate), you must set all displacements and all rotations to zero. 3. You can apply both forces and moments to nodes in an analysis.
Finally, in an analysis involving several beams connected together, you can connect the beams in two ways: 1. You can connect them with a pin joint, which forces the beams to move together at the connection, but allows relative rotation 2. You can connect them with a clamped joint, which forces the beams to rotate together at the connection.
In most FEA codes, you can create the joints by adding constraints, as discussed in Section 1.2.6 below. Occasionally, you may also wish to connect beam elements to solid, continuum elements in a model: this can also be done with constraints.Â
A good finite element code contains a huge library of different types of material behavior that may be assigned to elements. A few examples are described below.
The stress--strain law for the material may be expressed in matrix form as
Here, E
and v are Young’s modulus and
Poisson’s ratio for the material, while
The material behaves elastically until a critical stress (known as the yield stress) is reached. If yield is exceeded, the material deforms permanently. The yield stress of the matierial generally increases with plastic strain: this behavior is known as strain hardening.
The conditions necessary to initiate yielding under multiaxial loading are specified by a yield criterion, such as the Von-Mises or Tresca criteria. These yield criteria are built into the finite element code.
The strain hardening behavior of a material is approximated by allowing the yield stress to increase with plastic strain. The variation of yield stress with plastic strain for a material is usually specified by representing it as a series of straight lines, as shown in the picture.
Boundary conditions are used to specify the loading applied to a solid. There are several ways to apply loads to a finite element mesh:
Various symbols are used to denote displacement boundary conditions applied to a finite element mesh: a few of these are illustrated in the figure on the right. Some user-interfaces use small conical arrowheads to indicate constrained displacement components.
For example, to stretch a 2D block of material vertically, while allowing it to expand or contract freely horizontally, we would apply boundary constraints to the top and bottom surface as shown in the figure.
Observe that one of the nodes on the bottom of the block has been prevented from moving horizontally, as well as vertically. It is important to do this: the finite element program will be unable to find a unique solution for the displacement fields if the solid is free to slide horizontally.Â
During the analysis, the finite element program will
apply forces to the nodes with prescribed displacements, so as to cause them
to move to their required positions.Â
If only the
Difficulties arise if the user does not specify sufficient boundary constraints to prevent rigid body motion of a solid. This is best illustrated by example. Suppose we wish to model stretching a 2D solid, as described earlier. The examples to the right show two correct ways to do this.
The examples below show various incorrect ways to apply boundary conditions. In each case, one or more rigid body mode is unconstrained.
You may sometimes need to use more complicated boundary conditions than simply constraining the motion or loads applied to a solid. Some examples might be 1. Connecting different element types, e.g. beam elements to solid elements; 2. Enforcing periodic boundary conditions 3. Constraining a boundary to remain flat 4. Approximating the behavior of mechanical components such as welds, bushings, bolted joints, etc.
You can do this by defining constraints in an analysis.  At the most basic level, constraints can simply be used to enforce prescribed relationships between the displacements or velocities of individual nodes in the mesh. You can also specify relationships between motion of groups of nodes.
7.1.7 Contacting Surfaces and Interfaces
In addition to being subject to forces or prescribed displacements, solid objects are often loaded by coming into contact with another solid.
Modern finite element codes contain sophisticated
capabilities for modeling contact.Â
Unfortunately, contact can make a computation much more difficult,
because the region where the two solids come into contact is generally not
known a priori, and must be
determined as part of the solution.Â
This almost always makes the problem nonlinear
For this reason, many options are available in finite element packages to control the way contacting surfaces behave.
There are three general cases of contact that you may need to deal with: 1. A deformable solid contacts a stiff, hard solid whose deformation may be neglected. In this case the hard solid is modeled as a rigid surface, as outlined below. 2. You may need to model contact between two deformable solids 3. The solid comes into contact with itself during the course of deformation (this is common in components made from rubber, for example, and also occurs during some metal forming operations).
Whenever you model contact, you will need to 1. Specify pairs of surfaces that might come into contact. One of these must be designated as the master surface and the other must be designated as the slave surface. (If a surface contacts itself, it is both a master and a slave. Kinky!) 2. Define the way the two surfaces interact, e.g. by specifying the coefficient of friction between them.
In this case the stiffer of the two solids may be idealized as a rigid surface. Both 2D and 3D rigid surfaces can be created, as shown in the figure.
A rigid surface (obviously) can’t change its shape, but it can move about and rotate. Its motion is defined using a reference point on the solid, which behaves like a node. To move the solid around during an analyisis, you can define displacement and rotational degrees of freedom at this node. Alternatively, you could apply forces and moments to the reference point.  Finally, in a dynamic analysis, you can give the rigid solid appropriate inertial properties (so as to create a rigid projectile, for example).
This rather obscure finite element terminology refers to the way that contact constraints are actually applied during a computation. The geometry of the master surface will be interpolated as a smooth curve in some way (usually by interpolating between nodes). The slave surface is not interpolated. Instead, each individual node on the slave surface is constrained so as not to penetrate into the master surface. For example, the red nodes on the slave surface shown in the figure would be forced to remain outside the red boundary of the master surface.
For a sufficiently fine mesh, the results should not be affected by your choice of master and slave surface. However, it improves convergence (see below to learn what this means) if you choose the more rigid of the two surfaces to be the master surface. If you don’t know which surface is more rigid, just make a random choice. If you run into convergence problems later, try switching them over.
1. The contact formulation - `finite sliding’ or `small
sliding’ 2. You can specify the relationship between the contact
pressure and separation between the contacting surfaces. Alternatively, you
can assume the contact is `hard’ 3.
You can specify
the tangential behavior of the interface
7.1.8 Initial Conditions and external fields
For a dynamic analysis, it is necessary to specify the initial velocity and displacement of each node in the solid. The default value is zero velocity and displacement.
In addition, if you are solving a coupled problem
7.1.9 Solution procedures and time increments
The finite element method calculates the
displacement
You can use the same idea to simplify calculations involving deformable solids. In general, you should do so whenever possible. However, if either 1. You anticipate that material might stretch by more than 10% or so or 2. You expect that some part of the solid might rotate by more than about 10 degrees 3. You wish to calculate buckling loads for your structure you should account for finite geometry changes in the computation. This will automatically make your calculation nonlinear (and so more difficult), even if all the materials have linear stress-strain relations.
where M and K are called mass and stiffness matrices. Both M and K can be functions of u. There are 2.5 ways to integrate this equation.
1. The most direct method is called explicit time integration, or explicit dynamics and works something
like this. Remember that for a dynamic
calculation, the values of u and
The acceleration
can then be used to find the velocity
This procedure can then be applied repeatedly to march the solution through time. 2. The second procedure is called implicit time integration or implicit
dynamics. The procedure is very
similar to explicit time integration, except that instead of calculating the
mass and stiffness matrices at time t=0,
and using them to calculate acceleration at t=0, these quantities are calculated at time 3. The 2.5th method is called Modal Dynamics and only works if M and K are constant. In this case one can take the Fourier transform of the governing equation and integrate it exactly. This method is used to solve linear vibration problems.
The following guidelines will help you to choose the most appropriate method for your application:
1. For explicit
dynamics each time step can be calculated very fast. However, the method is stable only if 2. For implicit
dynamics the cost of computing each time step is much greater. The algorithm is unconditionally stable,
however, and will always converge even for very large 3. Modal Dynamics only works for linear elastic problems. It is used for vibration analysis.
where F() denotes
a set of b=1,2…N vector functions
of the nodal displacements
The nonlinear equations are solved using the
Newton-Raphson method, which works like this.Â
You first guess the solution to the equations
but of course it’s not possible to do this. So instead, take a
The result is a system of linear equations of the
form
In problems involving hard contact, an additional iterative method is used to decide
which nodes on the slave surface contact the master surface. This is just a brute-force method
The problem with any iterative procedure is that it
may not converge
The solution is (naturally) more likely to converge
if the guess
Convergence problems are the curse of FEM analysts. They are very common and can be exceedingly difficult to resolve. Here are some suggestions for things to try if you run into convergence problems: 1. Try applying the load in smaller increments. most commercial codes will do this this
automatically 2. Convergence problems are sometimes caused by ill conditioning in the stiffness
matrix. This means that the equations 3. Try to isolate the source of the problem. Convergence issues can often be traced to
one or more of the following: (i) Severe material nonlinearity; (ii) Contact
and (iii) Geometric nonlinearity. Try
to change your model to remove as many of these as possible 4. Convergence problems are often caused by some kind of mechanical or material failure in the solid, which involve a sudden release of energy. In this case, the shape of the solid may suddenly jump from one static equilibrium configuration to another, quite different, equilibrium configuration. There is a special type of loading procedure (called the Riks method) that can be used to stabilize this kind of problem. 5. Some boundary value problems have badly behaved governing equations. For example, the equations governing plane strain deformation of a perfectly plastic solid become hyperbolic for sufficiently large strains. Static FEM simply won’t work for these problems. Your best bet is to try an explicit dynamic calculation instead, perhaps using mass scaling to speed up the calculation.
In a nonlinear analysis, the solution may not converge if the load is applied in a single increment. If this is the case, the load must be applied gradually, in a series of smaller increments. Many finite element codes will automatically reduce the time step if the solution fails to converge.
The finite element method always calculates the displacement of each node in the mesh 1. Velocity and acceleration fields 2. Strain components, principal strains, and strain invariants,or their rates 3. Elastic and plastic strains or strain rates 4. Stress components; principal stresses; stress invariants 5. Forces applied to nodes or boundaries 6. Contact pressures 7. Values of material state variables (e.g. yield stresses) 8. Material failure criteria
All these quantities can be computed as functions of time at selected points in the mesh (either at nodes, or at element integration points); as functions of position along paths connecting nodes; or as contour plots.
7.1.11 Units in finite element computations
A finite element code merely solves the equations of
motion (or equilibrium), together with any equations governing material
behavior. Naturally, equations like F=ma and
7.1.12 Using Dimensional Analysis to simplify FEA analysis.
You may have used dimensional analysis to find relationships between data measured in an experiment (especially in fluid mechanics). The same idea can be used to relate variables you might compute in an FEA analysis (e.g. stress), to the material properties of your part (e.g. Young’s modulus) and the applied loading.
The basic idea is simple, and is best illustrated by
example. Suppose we wish to use FEA to
calculate the deflection of the tip of a cantilever with length L, Young’s modulus E and area moment of inertia I, which is subjected to a force P.Â
We would set this up as an FEA problem, entering data for L, E,
I, and P in the code, and computing                                                                 Â
If we
were asked to calculate the function f numerically,
we would have to run simulations where we vary E, I, L and P independently. This would be very
painful. Fortunately, since the relationship must be independent of the
system of units, we know we can re-write this expression so that both left
and right hand side are dimensionless
Now, we only need to calculate the function g. We could do this by keeping L and I fixed, and varying P to see the results of varying the first group; we could then keep P and L fixed and vary I to see the effect of varying the second group. The results could be displayed graphically as shown in the figure.
If we had done a linear analysis (no nonlinear geometric effects) the curves would be straight lines.
There is often more than one choice of dimensionless
group, and some are better than others.Â
For example, for the beam problem we could create a new dimensionless
group by multiplying together the two groups in the function g
This turns out to be a much better choice. In fact,
if we conducted a linear analysis we would find that the function h is independent of
Unfortunately, dimensional analysis alone will not
tell you the best dimensionless groups.Â
You have to use your physical intuition to identify them. For the beam example, you might remember
that E and I always appear as the product EI in the governing equations The beauty of using dimensional analysis to simplify numerical simulations is that, unlike in experiments, you don’t need to guess what variables influence the results. You know exactly what they are, because you typed them into the program!
The following steps (known as the Buckingham Pi theorem) will tell you how many dimensionless groups to look for: 1. List the variable you are computing, and also the variables you entered into the code to define the problem. Count the total number of variables and call it n 2. List the dimensions, in terms of fundamental units (i.e. mass, length, time, electric current, and luminous intensity) of all the variables 3. Count the number of independent fundamental units that appear in the problem (e.g. if
mass, length and time appear independently, then there are 3 different units)
and call the number k. Units are independent if they don’t always
appear in the same combination. For
example, in our beam problem mass and time are not independent, because they appear together as 4. A total of n-k independent dimensionless groups must appear in the dimensionless relationship. For the beam problem, we had 5 variables
7.1.13 Simplifying FEA analysis by scaling the governing equations
An alternative approach to identifying the dimensionless parameters that control the solution to a problem is to express the governing equations themselves in dimensionless form. This is a much more powerful technique, but is also somewhat more difficult to use.
We can illustrate the procedure using our beam problem again. Let x measure distance along the beam, and let w denote its vertical deflection. You may remember that linear Euler-Bernoulli beam theory gives the following governing equation for w
(the right hand side vanishes because no forces act on 0<x<L) while the boundary conditions are
(If you don’t remember these it doesn’t matter
We now re-write the equations so that they are
dimensionless. We aways start by
replacing all field variables (in this case w and x) with
dimensionless quantities. In this case
we could use
We now look and see if we can make further simplifications. Our objective is to remove as many material and geometric parameters from the equations as possible, by defining new dimensionless field variables or introducing dimensionless combinations of material or geometric variables. In this case, we see that if we define a new dimensionless displacement W so that
substitute, and cancel as many terms as possible, the governing equations become
In this form, the governing equations contain
absolutely no material or geometric parameters. The solution for W must therefore be independent of L,E,I or P. We can solve the equation just once, and
then work out the tip deflection from the value of W at
This scaling procedure is the best way to simplify numerical computations. It is more difficult to apply than dimensional analysis, however, and it is possible (although perhaps not a good idea) to run an FEA simulation of a problem where you don’t actually know the governing equations! In this case you should just use standard dimensional analysis to try to simplify the problem.
7.1.14 Dimensional analysis
It is good practice to scale a mechanics problem as
outlined in the preceding sections, and present results in dimensionless form.
Not all practicing engineers and managers are really comfortable with it,
however -   They don’t want to see data
presented in dimensionless form
The best way to deal with this when presenting
results in a report is to divide it into two sections
You can make dimensional analysis work in your
favor. It is not uncommon for your
boss to tell you to run a series of simulations where you vary a parameter
that can be shown on dimensional grounds to have absolutely no effect. Also, dimensional analysis often tells you
that varying two parameters are equivalent
|
|||||||||||||||||||||||||
|
(c) A.F. Bower, 2008 |
 Plane
Stress Finite Element Mesh : A plane stress finite element mesh is used
to model a plate - like solid which is loaded in its own plane. The solid must have uniform thickness, and
the thickness must be much less than any representative cross sectional
dimension. A plane stress finite
element mesh for a thin plate containing a hole is shown in the figure to the
right. Only on quadrant of the
specimen is modeled, since symmetry boundary conditions will be enforced
during the analysis.
