Chapter 8

 

Theory and Implementation of the Finite Element Method

 

 

 

The derivation and implementation of the finite element method outlined in the previous chapter is simple and easy to follow, but it gives the misleading impression that the finite element method relies on the principle of minimum potential energy, and so is applicable only to linear elastic solids.  This is not the case, of course  the finite element method can solve problems involving very complex materials and large shape changes.

 

This chapter contains

  1. A more rigorous derivation of the finite element equations, based on the principle of virtual work, which was derived in Section 2.4.
  2. A more sophisticated implementation of finite element method for static linear elasticity. This includes more accurate element interpolation schemes, and also extends the finite element method to three dimensions.
  3. A discussion of time integration schemes that are used in finite element simulations of dynamic problems, and a discussion of modal techniques for dynamic linear elasticity problems;
  4. An extension of the finite element method to nonlinear materials, using the hypoelastic material model described in Section 3.2 as a representative nonlinear material;
  5. An extension of the finite element method to account for large shape changes, using finite strain elasticity as a representative example;
  6. A discussion of finite element procedures for history dependent solids, using small strain viscoplasticity as a representative example.
  7. A discussion of the phenomenon of `locking’ that can cause the standard finite element method to fail in certain circumstances.   Several techniques for avoiding locking are presented.

 

In addition, a set of sample finite element codes (implemented in MAPLE and MATLAB) are provided to illustrate the how the various finite element procedures are implemented in practice.

 

 

8.1 Generalized FEM for static linear elasticity

 

This section gives a more general derivation and implementation of the finite element method for static linear elastic solids than the energy-based derivation given in Chapter 7.

 

8.1.1 Review of the principle of virtual work

 

Governing equations: We begin by summarizing the usual governing equations of linear elasticity, which must be solved by the FEA code.  

 

Given:

1.       The shape of the solid in its unloaded condition  

2.       The initial stress field in the solid (we will take this to be zero in setting up our FEM code)

3.       The elastic constants for the solid  

4.       The thermal expansion coefficients for the solid, and temperature distribution (we will take this to be zero for our FEM code, for simplicity)

5.       A body force distribution  acting on the solid (Note that in this section we will use b to denote force per unit volume rather than force per unit mass, to avoid having to write out the mass density all the time)

6.       Boundary conditions, specifying displacements  on a portion  or tractions on a portion  of the boundary of R

 

Calculate displacements, strains and stresses  satisfying the governing equations of static linear elasticity

1.       The strain-displacement equation  

2.       The elastic stress-strain law  

3.       The equation of static equilibrium for stresses  

4.       The boundary conditions on displacement and stress  

 

The principle of virtual work: As we discussed in section 2.4, the principle of virtual work can be used to replace the stress equilibrium equations.  

 

To express the principle, we define a kinematically admissible virtual displacement field , satisfying   on .  You can visualize this field as a small change in the displacement of the solid, if you like, but it is really just an arbitrary differentiable vector field.  The term `kinematically admissible’ is just a complicated way of saying that  on  - that is to say, if you perturb the displacement slightly, the boundary conditions on displacement are still satisfied.

 

In addition, we define an associated virtual strain field

 

The principle of virtual work states that if the stress field  satisfies

 

for all possible virtual displacement fields and corresponding virtual strains, it will automatically satisfy the equation of stress equilibrium , and also the traction boundary condition  

 

 

8.1.2 Integral (weak) form of the governing equations of linear elasticity

 

The principle of virtual work can be used to write the governing equation for the displacement field in a linear elastic solid in an integral form (called the `weak form’).  Instead of solving the governing equations listed in the preceding section, the displacements, strains and stresses  are calculated as follows. 

1.       Find a displacement field  satisfying

 

for all virtual velocity fields  satisfying  on .

2.       Compute the strains from the definition  

3.       Compute the stresses from the stress-strain law  

The stress will automatically satisfy the equilibrium equation and boundary conditions, so all the field equations and boundary conditions will be satisfied.

 

The significance of this result is that it replaces the derivatives in the partial differential equations of equilibrium with an equivalent integral, which is easier to handle numerically.  It is essentially equivalent to replacing the equilibrium equation with the principle of minimum potential energy, but the procedure based on the principle of virtual work is very easily extended to dynamic problems, other stress-strain laws, and even to problems involving large shape changes.

 

Derivation: start with the virtual work equation

 

Recall that , and that , so that

 

Finally, recall that  and that the elastic compliances must satisfy  so that .  Finally, this shows that

 

Substituting into the virtual work equation gives the result we need.

 

 

 

8.1.3 Interpolating the displacement field and the virtual velocity field

 

To solve the integral form of the elasticity equations given in 8.1.2, we discretize the displacement field.  That is to say, we choose to calculate the displacement field at a set of n discrete points in the solid (called `nodes’ in finite element terminology).  We will denote the coordinates of these special points by , where the superscript a ranges from 1 to N.  The unknown displacement vector at each nodal point will be denoted by .

 

The displacement field at an arbitrary point within the solid will be specified by interpolating between nodal values in some convenient way.  An efficient and robust implementation of the finite element method requires a careful choice of interpolation scheme, but for now we will denote the interpolation in a general way as

 

Here, x denotes the coordinates of an arbitrary point in the solid.  The interpolation functions  are functions of position only, which must have the property that

 

for all b=1…N(This is to make sure that the displacement field has the correct value at each node).  Recently developed meshless finite element methods use very complex interpolation functions, but the more traditional approach is to choose them so that

 

The simple constant strain triangle elements introduced in 7.1 are one example of this type of interpolation scheme.  We will define more complicated interpolation functions shortly.

 

We can obviously interpolate the virtual velocity field in exactly the same way (since the principle of virtual work must be satisfied for all virtual velocities, it must certainly be satisfied for an interpolated velocity field…) so that

 

where  are arbitrary nodal values of virtual velocity.

 

 

8.1.4 Finite element equations

 

Substituting the interpolated fields into the virtual work equation, we find that

 

where summation on a and b is implied, in addition to the usual summation on i,j,k,l

 

Note that the interpolation functions are known functions of position. We can therefore re-write the virtual work equation in matrix form as

 

where

 

Here K is known as the `stiffness matrix’ and f is known as the force vector.  K is a function only of the elastic properties of the solid, its geometry, and the interpolation functions and nodal positions. It is therefore a known matrix.  Similarly, f is a function only of the known boundary loading and body force field, and the interpolation scheme and nodal positions.  Observe that the symmetry of the elasticity tensor implies that K also has some symmetry  specifically .

 

The virtual work equation must be satisfied for all possible sets of  with  for nodes a that lie on .   At these nodes, the displacements must satisfy .   Evidently, this requires

 

This is a system of n linear equations for the n nodal displacements.

 

 

8.1.5 Simple 1D Implementation of the finite element method

 

Before describing a fully general 3D implementation of the finite element method, we will illustrate all the key ideas using a simple 1-D example. Consider a long linear elastic bar, as shown in the picture.  Assume

1.       The bar has shear modulus  and Poisson’s ratio  

2.       The bar has cross section  and length L

3.       It is constrained on all its sides so that  

4.       The bar is subjected to body force ,

5.       The bar is either loaded or constrained at its ends, so that the boundary conditions are either   or displacement  at x=0 and x=L

 

For this 1-D example, then, the finite element equations reduce to

 

where

 

We could obviously choose any interpolation scheme, evaluate the necessary integrals and solve the resulting system of equations to compute the solution.  It turns out to be particularly convenient, however, to use a piecewise-Lagrangian interpolation scheme, and to evaluate the integrals numerically using a Gaussian quadrature scheme.

 

To implement the Lagrangian interpolation scheme, we sub-divide the region  into a series of elements, as illustrated in the figure.  Each element is bounded by two nodal points, and may also contain one or more interior nodes. The displacement field within the element is interpolated between the nodes attached to the element.  So, we would use a linear interpolation between the nodes on a 2-noded element, a quadratic interpolation between the nodes on a 3 noded element, and so on.

Linear 1-D element

 

Quadratic 1-D element

 

 

Generic linear and quadrilateral 1-D elements are illustrated in the table.  The local nodes on the element are numbered 1 and 2 for the linear element, and 1,2,3 for the quadratic element as shown.  We suppose that the element lies in the region .  The displacements within the element are then interpolated as

 

where  denotes the number of nodes on the element,  denotes the value of the displacement at each node, and the shape functions are given in the table.                

                             
Of course, the actual nodal coordinates do not lie at 1, +1 and 0 for all the elements.  For a general element, we map this special one to the region of interest.  A particularly convenient way to do this is to set

 

where  denotes the coordinate of each node on the element, and  is the number of nodes on the element (2 or 3).  Elements that interpolate displacements and position using the same shape functions are called isoparametric elements.

 

Next, we need to devise a way to do the integrals in the expressions for the stiffness matrix and force vector.  We can evidently divide up the integral so as to integrate over each element in turn

 

where  is the total number of elements, and  and  denote the coordinates of the ends of the lth element.  We now notice an attractive feature of our interpolation scheme.  The integral over the lth element depends only on the shape functions associated with the nodes on the lth element, since the displacement in this region is completely determined by its values at these nodes.  We can therefore define element stiffness matrix, and element force matrix

 

for each element, which depend on the geometry, interpolation functions and material properties of the element.  The first and last elements have additional contributions to the element force vector from the boundary terms .  The global stiffness matrix is computed by summing all the element stiffness matrices

 

 

Finally we need to devise a way to compute the integrals for each element stiffness matrix.  It is convenient to map the domain of integration to [-1,+1] and integrate with respect to the normalized coordinate  - thus

 

where  is the Jacobian associated with the mapping, which may be computed as

 

1-D integration points and weights

M=1

 

M=2

 

M=3

 

 

Note that the mapping also enables us to calculate the shape function derivatives in the element stiffness matrix as

 

 

Finally, note that integrals may be computed numerically using a quadrature formula, as follows

 

where    I=1…M denotes a set of integration points in the region [-1,+1], and  is a set of integration weights, which are chosen so as to make the approximation as accurate as possible. Values are given in the table to the right for  and 3. Higher order integration schemes exist but are required only for higher order elements.  For the linear 1-D element described earlier a single integration point is sufficient to evaluate the stiffness exactly. Similarly, for the quaratic element, two integration points will suffice.

 

 

8.1.6 Summary of the 1D finite element procedure

 

To summarize, then, the finite element solution requires the following steps:

1.       For each element, compute the element stiffness matrix as follows:

 

where

             

and the integration points  are tabulated above, and shape functions  were listed earlier.

2.       Assemble the contribution from each element to the global stiffness

 

3.       Similarly, if there is a non-zero body force, then compute for each element

 

and assemble the global force vector

 

4.       Add contributions to the force vector from prescribed traction boundary conditions at  and  

 

where the  superscript denotes the node that lies at x=L.

5.       Modify the stiffness matrix to enforce the constraints

 

6.       Solve the system of linear equations

 

for the unknown displacements  

 

 

 

 

8.1.7 Example FEM Code and solution

 

 

 

 

 

 

A simple example MAPLE code for this 1-D example can be found in the file FEM_1D_Static.mws

 

It is set up to solve for displacements for a bar with the following parameters:

1.       Length L=5, unit x-sect area,

2.       Shear modulus 50, Poisson’s ratio 0.3,

3.       Uniform body force magnitude 10,

4.       Displacement u=0 at x=0

5.       Traction t=2 at x=L.

 

The code computes the (1D) displacement distribution in the bar. The predicted displacement field is plotted on the right.

 

Of course in general we want to calculate more than just displacements  usually we want the stress field too. We can calculate the stress field anywhere within an element  by differentiating the displacements to calculate strains, and then substituting into the constitutive relation.  This gives

 

This works well for a uniform body force with quadratic (3 noded elements) as the plot on the right shows.

 

However, if we switch to linear elements, the stress results are not so good (displacements are still calculated exactly).  In this case, the stress must be uniform in each element (because strains are constant for linear displacement field), so the stress plot looks like the figure to the right.


Notice that the stresses are most accurate near the center of each element (at the integration point).  For this reason, FEM codes generally output stress and strain data at integration points. 

 

It is interesting also to examine the stiffness matrix (shown below for 3 linear elements, before addition of the u=0 constraint for the first node )

 

Notice that stiffness is symmetric, as expected, and also banded.  A large FEM matrix is sparse  most of the elements are zero.  This allows the matrix to be stored in compact form  for very large matrices indexed storage (where only the nonzero elements together with their indices are stored) is the best approach; for smaller problems skyline storage or band storage (where only the central, mostly nonzero, band of the matrix is stored) may be preferable.  In this case equation numbers need to be assigned to each degree of freedom so as to minimize the bandwidth of the stiffness matrix.

 

 

 

8.1.8 Extending the 1D finite element method to 2 and 3 dimensions

 

It is straightforward to extend the 1-D case to more general problems.  All the basic ideas remain the same.   Specifically

1.       In both 2D and 3D we divide up our solid of interest into a number of elements, shown schematically for a 2D region in the picture on the right.

2.       We define interpolation functions  for each element in terms of a local, dimensionless, coordinate system within the element.  The coordinates satisfy .  The displacement field and the position of a point inside an element are computed in terms of the interpolation functions as

 

where  denote the shape functions,  denote the displacement values and coordinates of the nodes on the element, and  is the number of nodes on the element.

3.       We introduce an element stiffness matrix for each element by defining

 

where  denotes the element stiffness matrix for the (lth) element, and  denotes the volume (in 3D) or area (in 2D) of the (lth) element, while  denotes the surface of the (lth) element

4.       The volume integrals over each element are calculated by expressing the volume or surface integral in terms of the dimensionless coordinates , and then evaluating the integrals numerically, using a quadrature formula of the form

 

Here,  are a set of  integration weights (just numbers), and  are a set of coordinates that are selected to make the integration scheme as accurate as possible (also just numbers).

5.       The global stiffness matrix

 

is then computed by summing the contribution from each element as

 

6.       The stiffness matrix is modified to enforce any prescribed displacements

7.       The system of equations

 

is solved for the unknown nodal displacements.

8.       The stresses and strains within each element are then deduced.

 

To implement this procedure, we must (a) Define the element interpolation functions; (b) Express the integrals for the element stiffness matrices and force vectors in terms of normalized coordinates; (c) Formulate a numerical integration scheme to evaluate the element stiffness matrices and force vectors.

These details are addressed in the sections to follow.

 

 

 

8.1.9 Interpolation functions for 2D elements

 

The 2D interpolation functions listed below are defined for the region

 

The numbers shown inside the element show the convention used to number the element faces.

 

2D interpolation functions

 

 

 

 

 

                                           

 

 

8.1.10 Interpolation Functions for 3D elements

 

The 3D interpolation functions listed below are defined for the region  

                                         

3D Interpolation Functions

 

 

 

 

 

    

The element faces are numbered as follows.

 

Linear and quadratic tetrahedral

 

Face 1 has nodes 1,2,3

Face 2 has nodes 1,4,2
Face 3 has nodes 2,4,3
Face 4 has nodes 3,4,1

 

Linear and quadratic brick elements

 

Face 1 has nodes 1,2,3,4

Face 2 has nodes 5,8,7,6

Face 3 has nodes 1,5,6,3

Face 4 has nodes 2,6,7,3

Face 5 has nodes 3,7,8,4

Face 6 has nodes 4,8,5,1

 



 

8.1.11 Volume integrals for stiffness and force in terms of normalized coordinates

 

In this section we outline the procedure that is used to re-write the integrals for the element stiffness and force in terms of the normalized coordinates .  The integrals are

 

To evaluate them, we need to

1.       Find a way to calculate the derivatives of the shape functions in terms of  

2.       Map the volume (or area) integral to the region  

 

Calculating the shape function derivatives. The shape function derivatives can be evaluated by writing

 

where the derivatives  are easy to compute (just differentiate the expressions given earlier…).  To compute  recall that the coordinates of a point at position  within an element can be determined as

 

where  denotes the number of nodes on the element. Therefore

 

Note that  is a 2x2 matrix (in 2D) or a 3x3 matrix (in 3D).  Finally,  follows as the inverse of this matrix

 

 

Mapping the volume integral: To map the region of integration we define

 

where the matrix  was defined earlier.  Then the integral with respect to x is mapped into an integral with respect to  by setting

 

We note in passing that the boundary integral in the element force vector can be regarded as a 1-D line integral for 2D elements and a 2D surface integral for 3D elements.  So the procedures we developed in 8.1.5 (1D elements) can be used to evaluate the surface integral for a 2D element.  Similarly, the procedures we develop to integrate stiffness matrices for 2D elements can be used to evaluate the surface integral for a 3D element.

 

 

 

8.1.12 Numerical integration schemes for 2D and 3D elements

 

Finally, to evaluate the integrals, we once again adopt a quadrature scheme, so that

 

The integration points  and weights  depend on the element geometry, and are listed below for a few common element types

 

Integration points for triangular elements

 

1 point 

 

3 point 

 or  

(the first scheme here is optimal, but has some disadvantages for quadratic elements because the integration points coincide with the midside nodes.  The second scheme is less accurate but more robust).

4 point

 

 

 Integration points for tetrahedral elements

 

1 point

 

 

4 point

 

 

where  

 

 

Quadrilateral and hexahedral elements

 

For quadrilateral elements we can simply regard the integral over 2 spatial dimensions as successive 1-D integrals

 

which gives rise to the following 2D quadrature scheme:  Let  and  for I=1…M denote 1-D quadrature points and weights listed below. Then in 2D, an  quadrature scheme can be generated as follows:

for J=1…M and K=1…M    let    

Similarly, in 3D, we generate an  scheme as:

for J=1…M , K=1…M  L=1…M   let

 

M=1

 

 

M=2

 

 

M=3

 

 

 

Choosing the number of integration points: There are two considerations.  If too many integration points are used, time is wasted without gaining any accuracy).  If too few integration points are used, the stiffness matrix may be singular, or else the rate of convergence to the exact solution with mesh refinement will be reduced.  The following schemes will avoid both

 

Number of integration points for fully integrated elements

Linear triangle (3 nodes):  1 point

Quadratic triangle (6 nodes): 4 points

Linear quadrilateral (4 nodes): 4 points

Quadratic quadrilateral (8 nodes): 9 points

Linear tetrahedron (4 nodes): 1 point

Quadratic tetrahedron (10 nodes): 4 points

Linear brick (8 nodes): 8 points

Quadratic brick (20 nodes): 27 points

 

There are situations where it is preferable to use fewer integration points and purposely make the stiffness singular.   These are discussed in more detail in Section 8.5.

 

 

 

8.1.13 Summary of formulas for element stiffness and force matrices

 

With these definitions, then, we write the element stiffness matrix as

 

where

                         

 

 

 

8.1.14 Sample 2D/3D linear elastostatic FEM code

 

You can find a MAPLE implementation of a simple 2D/3D static linear elasticity code in the file   FEM_2Dor3D_linelast_standard.mws

 

The code reads an input file.  Several examples are provided :

1.       Linear_elastic_triangles.txt: Simple 2D plane strain problem with two triangular elements

2.       Linear_elastic_quad4.txt: Simple 2D plane strain problem with eight 4 noded quadrilateral elements

3.       Linear_elastic_quad8.txt: Simple 2D plane strain problem with two 8 noded quadrilateral elements

4.       Linear_elastic_brick4.txt: Simple 3D problem with 8 noded brick elements

No._material_props:    3

    Shear_modulus:   10.

    Poissons_ratio:  0.3
    Plane strain/stress: 1

No._coords_per_node:   2

No._DOF_per_node:      2

No._nodes:             4

Nodal_coords:

    0.0   0.0

    1.0   0.0

    1.0   1.0

    0.0   1.0

No._elements:                       2

Max_no._nodes_on_any_one_element:   3

element_identifier; no._nodes_on_element; connectivity:

    1  3  1 2 4

    1  3  2 3 4

No._nodes_with_prescribed_DOFs:  3

Node_#, DOF#, Value:

   1 1 0.0

 

 

As an example, we show how to run the program with the first input file. The file sets up the problem illustrated in the figure above. The elements are linear elastic plane strain with

 

The program input file is listed on the right. Here is a brief explanation of the data in the file

1.       The first part of the input file specifies material properties.  A number ‘1’ on the Plane strain/stress line indicates a plane strain analysis; a number ‘0’ indicates plane stress.

2.       The second part specifies properties and coordinates of the nodes.  For a 2D problem each node has 2 coordinates and 2 DOF; for a 3D problem each node has 3 coordinates and 3DOF.  Then enter nodal coordinates for each node.

3.       The third part lists the element properties.  Here, you must specify the number of elements, and the maximum number of nodes on any one element (you can mix element types if you like).  Then you must specify the nodes connected to each element (known as element connectivity).   For each element, you must specify the number of nodes attached to the element; an identifier that specifies the element type (you can enter any number in this version of the code  the identifier is provided to allow addition of more sophisticated element types such as reduced integration elements), then enter the nodes on each element following the convention shown earlier.

4.       The fourth part of the file specifies boundary constraints.  For any constrained displacements, enter the node number, the displacement component to be prescribed, and its value.

5.       The last part of the file specifies distributed loading acting on the element faces.  The loading is assumed to be uniform.  For each loaded boundary, you should specify the element number, the face of the element (the face numbering convention was described in section 7.2.9 and 7.2.10  note that you must be consistent in numbering nodes and faces on each element), and the components of traction acting on the element face, as a vector with 2 or 3 components.

 

Note that the program performs absolutely no error checking on the input file.  If you put in a typo, you will get some bizzarre error message from MAPLE  often during element stiffness assembly.

 

For the input file shown, the program produces an output file that looks like this

The code prints the displacements at each node in the mesh, and also the strains and stresses at each integration point (where these quantities are most accurate)  for each element.

 

To run the code, you must complete the following steps

1.       Open the maple executable file;

1.       Edit the code to insert the full path for the input file in the line near the top of the code that reads

> # Change the name of the file below to point to your input file

> infile :=fopen(`D:/fullpathoffile/Linear_elastic_triangles.txt`,READ):

2.       Scroll down near the bottom to the line that reads

> #      Print nodal displacements, element strains and stresses to a file

> #

> outfile := fopen(`path/Linear_elastic_triangles.out`,WRITE):

and enter a name for the output file.

3.       Return to the top of the file, and press <enter> to execute each MAPLE block. You will see the code plot the undeformed and deformed finite element mesh at the end.  The stresses and strains in the elements are printed to the output file.

 

 

 

(c) A.F. Bower, 2008
This site is made freely available for educational purposes.
You may extract parts of the text
for non-commercial purposes provided that the source is cited.
Please respect the authors copyright.