The following content is provided under a Creative
Commons license.
Your support will help MIT OpenCourseWare continue to
offer high-quality educational resources for free.
To make a donation or view additional materials from
hundreds of MIT courses visit MIT OpenCourseWare at
ocw.mit.edu.
PROFESSOR: Ladies and gentlemen, welcome to this
lecture on nonlinear finite element analysis of solids and
structures.
In this lecture I'd like to discuss with
you structural elements.
Structural elements are, of course, employed to model
beam, plate and shell structures and are most
important elements.
Because of their importance in engineering practice much
research and development effort has been focused on the
development of efficient structural elements.
In this and the next lecture I'd like to discuss with you
some modern effective elements.
We will first discuss shell elements and then beam
elements and then we go back to use the shell elements, a
concept that we discussed in some actual applications.
When we do structural analysis we should keep one method in
mind, namely that in a geometrically nonlinear
analysis, a flat shell, referred to as a plate, goes
very rapidly over into the behavior of a shell because of
the curvature that develops as the plate deforms.
Therefore, to analyze geometrically nonlinear plates
we really are quite well off using general shell elements.
And I'd like to now focus our attention on the development
of general shell elements that we actually then employ to
analyze plates as well as general shells.
There are various solution approaches that one can follow
for the development of efficient elements.
And one such approach is the use of general
beam and shell theories.
I'm thinking of beams as well as shells although I want to
focus our attention on shells, really, in this first lecture.
One starts with beam or shell theory as general as possible
and develops the governing differential equations.
From the governing differential equation one
develops variational formulations and one
discretizes those variation formulations using finite
element interpolations.
This is the approach that is taken.
The disadvantage of that approach is, in general, lack
of generality of the approach.
You're starting off with a particular shell
theory, beam theory.
You of course would like to have that shell theory as
general as possible but you will find that really, the
shell theory that you're starting of will mostly only
be applicable to a certain class of shells.
Therefore your finite elements that you're developing would
also be only applicable to that same class of shells.
And that means in engineering practice, in actual usage, the
user has to be very familiar for which the particular
element developed, as shown here.
I'll discuss now for what kinds of shells this
particular shell element is really applicable.
We would rather like to have shell elements that are
applicable to any shell.
Of course this is a very big aim, very
difficult to achieve.
But this is what we would like to have ideally
in engineering practice.
The other difficulty with this approach is that frequently a
large number of nodal degrees of freedom have to be carried
along in the development of the shell elements.
And what I'm thinking of there is that you don't just have
translations and rotations at the nodal points, which has
engineering degrees of freedom that we would like to have and
see in for the element, but you also have to have
additional degrees of freedoms relating to the curvatures in
the elements.
And so on.
So this of course would mean, or does mean, difficult use of
such elements and these reasons, these two reasons
here have really driven the research and development
efforts in different directions.
Another approach is to use simple elements.
Simple elements, but a large number of elements, then to
model very complex beam and shell structures.
As an example I'd like to just refer you to a 3-node
triangle, a flat element in which the plate-bending
behavior is modeled in a particular way and the plane
stress behavior is modeled as a constant strain, constant
stress element.
These two are superimposed, these two behaviors are
superimposed and you have a very simple shell element that
in certain analyses can be quite effective.
Of course we have to recognize in this approach that the
coupling between the membrane and bending action is only
introduced at the element nodes.
That is a major disadvantage.
And that is the reason why you need so many elements to model
a shell and that if we use a triangular 3-noded element
with just a constant strain, constant stress element to
model the membrane behavior, the membrane action, of course
the membrane action is quite poorly approximated.
And that is another reason why we need so many elements to
model a complex shell behavior.
Here on this viewgraph I'm showing a picture of the
element that I just referred to.
Here you have a triangular element in the three
dimensional space.
Notice we introduce a local coordinate system, x bar 2, x
bar 3, x bar 1.
Local coordinate system, and in this local coordinate
system we measure the displacements and rotations.
And we superimpose for this element the bending behavior,
the bending behavior corresponding to this degree
of freedom, that degree of freedom and this degree of
freedom at every node, of course.
We add, or superimpose onto this bending behavior the
membrane behavior which corresponds to these two
degrees of freedom.
And we immediately notice that corresponding to this degree
of freedom we don't have a real physical stiffness and we
introduce a little artificial stiffness as shown down here.
Now this artificial stiffness has to be selected and you
want to select it such as to take out the singularity out
of the system but yet make the stiffness not too big so as to
destroy the behavior of the element.
Because it's an artificial stiffness you really want to
make it as small as possible just to take out the
singularity out of this element when you apply this
element in the modeling of general shell structures.
This artificial stiffness actually is quite bothersome
in nonlinear analysis.
It can provide problems and we really don't like it.
But if we use this approach we have to introduce it and well,
we have to, so to say, live with it, with the difficulties
that we encounter.
But the other approach that I want to discuss with you
really quite extensively in these two lectures, namely
using the isoparametric elements, having curved
elements there as well, we don't introduce this
artificial stiffness anymore because our experiences of
introducing it in nonlinear analysis show us that there
are many difficulties that come into the analysis
procedure if you have this artificial stiffness.
So we got rid of it.
We don't need to use it any longer for the more modern
elements that I will be talking about just now.
The approach for these modern elements is to use
isoparametric interpolations and we talk then about the
isoparametric (degenerate) beams and shell elements.
"Degenerate" because we degenerate these elements, or
we obtain these elements I should say, by degeneration
from three dimensional behavior.
We will talk much more about it just now.
But in essence we are saying we take the 3-D continuum
equations and we degenerate those equations to the
particular shell behavior and beam behavior for beams that
we would like to capture.
The resulting elements can be used to model quite general
beam and shell structures.
And that is, of course, a very large advantage in engineering
practice if you can use the same elements to model a
variety of structures.
The basic approach of this isoparametric interpolation is
to use the total and updated Lagrangian formulations that
we developed earlier.
We talked in the earlier lectures quite extensively
about the total updated Lagrangian formulation, the
continuum mechanics equations, as well as the finite element
discretization of the continuum mechanics equations.
But we applied the final discretization only to 2-D and
3-D solid elements.
Now we want to do the same for shell elements.
We recall that in the T.L. formulation the governing
equation is this one here, which is nothing else than the
principal of virtual work operating on the second
Piola-Kirchhoff stress and the variation on the
Green-Lagrange strain.
This integral has taken over the original volume of the
structure, of the element, when we
develop a finite element.
And this of course, the internal virtual work, and
here we have the external virtual work.
Notice the linearization of this left integral here
resulted into these three integrals.
We went through that linearization in quite some
detail and we talked about the individual terms.
I don't think it's now necessity to review that
material anymore.
Please refer to the earlier lectures.
The same approach of course we used also for the U.L.
formulation.
Here is the general starting point, the principle of
virtual work now, using second Piola-Kirchhoff stresses refer
to the configuration at time t.
Variations in the Green-Lagrange strains refer
to the time configuration at time t.
This gives the internal virtual work corresponding to
time t plus delta t, t plus delta t.
And this is the external virtual work, same external
virtual work of course that we are having in the total
Lagrangian formulation.
The linearization of the left hand side integral here
results into these three integrals.
Once again we talked about the linearization quiet
extensively and if you refer to the earlier lectures surely
you recognize individual terms that you're seeing here now.
We use these governing equations for the total
Lagrangian and updated Lagrangian formulation to
develop the general shell elements.
And what we have to do now is to impose on these equations
the basic assumptions of beam and shell action.
And let us go now through these basic assumptions one by
one carefully.
The first assumption is that the material particles
originally on a straight line normal to the mid-surface of
the beam or the shell remain on that straight line
throughout the response history.
This is one most important assumption.
You must have encountered this assumption or at least some
form of it already earlier in your discussion of beam
theories and possibly shell theories.
Let's look at this assumption more closely, so.
For beams we would say plane sections initially normal to
the mid-surface remain plane sections during
the response history.
This is basically saying the same thing
what I just said earlier.
And if you look at this closely you recognize that we
do not say that the plane sections initially normal to
the mid-surface remain plane sections during the response
history and remain normal to the mid-surface.
We don't say that.
That's of course being said when you use the
Euler-Bernoulli beam theory.
We don't say this, that the plane sections remain normal
to the mid-surface throughout the response history.
We don't say that and because we don't say that we in effect
include in an approximate way shear deformations.
In other words, we look here at the effect of transverse
shear deformations is included, and hence the lines
initially normal to the mid-surface do not remain
normal to the mid-surface during the deformations.
Let's look at what this means pictorially.
Here we have a section of a beam at time 0 and we draw a
line normal, that is, at 90 degrees to the mid-surface,
shown as a dashed line.
And we identify particles on that line.
Here we have four such [? rad ?]
material particles.
Now the beam will move, deform, go through large
displacements, large rotations.
But actually we assume small strains.
And we see that these material particles which were
originally up here are now down here.
We identify that these material particles are still
on a straight line.
But this straight line is not anymore normal, that it is at
90 degrees to the mid-surface.
And because it is not any more normal to the mid-surface we
do include shear deformations approximately because we
assume that the shear deformations are constant
throughout the thickness of the beam.
This is a most important assumption.
We're looking here what looks like a beam but actually, if
you think of another dimension here, you can directly see
that the same picture is also applicable to
the motion of a shell.
The second important assumption is that the stress
in the direction normal to the beam or shell mid-surface is
zero throughout the response history.
In other words, there is no stress developed normal to the
mid-surface.
But notice that here is a stress along the material
fiber that is initially normal to the mid-surface is
considered.
Now this material fiber which is initially normal to the
mid-surface will not remain normal to the
mid-surface as I just said.
And in the motion we will consider always this stress in
the direction of that material fiber which was originally
normal to the mid-surface.
So after motion has taken place we are not really
talking anymore exactly--
you want to look in great detail at what's happening--
we don't talk anymore exactly about the stress, that is
normal to the current mid-surface.
But we always talk about the stress in the direction of the
fiber that was initially normal to the mid-surface.
That's being said here.
And the third assumption, also most important assumption, is
that the thickness of the beam or shell remains constant.
Here then we clearly identify that we are using really a
small-- we are assuming small strain conditions, but we
allow for very large displacements and rotations.
Well, with these three kinematic and static
assumptions clearly identified we are now ready to actually
develop the shell element interpolations.
And let's go at that.
The first point is that we incorporate the geometric
assumptions.
Straight lines normal to the mid-surface remain straight,
put here in quotes, that geometric assumption and the
geometric assumption that the shell thickness remains
constant throughout the whole motion.
These were two assumptions that we just discussed.
We incorporate that into our shell element formulation by
using the appropriate geometric and displacement
interpolations.
We incorporate the condition of zero stress normal to the
mid-surface, I put it in quotes here, because remember,
we are talking about the stress in the direction of the
fiber that was originally normal to the mid-surface.
We incorporate this condition by using the appropriate
stress-strain law.
Let's talk first about this assumption and then about this
assumption, how we're using these to actually develop our
shell elements.
To focus our attention I'd like to talk
about a 9-node element.
However.
we will later on see that in practice actually we don't use
the 9-node element very much.
We actually recommend the use of a 16-node element and a
4-node element but this 9-node element in some
analysis is also used.
And it certainly is an element with which I can discuss with
you, share with you all the experiences regarding the
formulation of the elements because what we're talking
about now really is applicable to any of the elements.
In fact, we're talking about variable number nodes
elements, where the number of nodes can be selected by the
analyst and the geometric assumptions that we're now
talking about are the same for any one of these elements.
How do we go about the formulation?
Well, one important point is that we introduce at each node
lying on the mid-surface, and here we see such 9-nodes, a
director vector, a director vector t v n k, t referring
already to the geometry at time t.
Of course this director vector is actually input by the
analyst for time 0 and then it evolves with the
motion of the shell.
Also we're introducing for the analysis, and that's being
done automatically in the computer program, these two
vectors here, t v 1 k and t v 2 k, which are normal to the
director vector.
These vectors are calculated automatically in
the computer program.
We talk more about it a little later.
Notice that the thickness here at this node is a k, and
notice that v n k at node k-- k of course
stands for that node--
acts into the direction off the thickness here.
Notice that such [? triad ?]
of vectors is of course being worked with at
each of these nodes.
And notice that the thickness at the nodes can change.
The element is defined as follows.
As far as the analyst is concerned the initial nodal
point coordinates of all the nodal points on the
mid-surface must be input.
Also the initial director vector must be input, here now
you see the zero, and the thickness at every
node must be input.
Notice if these director vectors at all of the nodes
are known, with the thicknesses at the nodes of
course, then we can interpolate the thickness at
any point of the mid-surface of the shell and we can
interpolate the director vector corresponding to any
point on the mid-surface.
Here such point on the mid-surface we get the
thickness at that point, from the thicknesses that we have
here, and from the director vectors.
And of course we are also getting the director vector at
this point from these director vectors.
So the analyst must put in the nodal point coordinates of the
mid-surface nodes and the direction cosines of these
director vectors.
Much of it of course can be generated
in a practical analysis.
We use an isoparametric coordinate system with
coordinates r, s, and t.
The coordinates r and s correspond to a measure in the
mid-surface.
The coordinate t is measured in the direction of the
director vectors.
The geometry at time 0 is interpolated as shown here in
this equation.
0 x i gives us the coordinates, three, i goes
from one to three, of any material particle in the
stationary coordinate frame.
I should point out once more very strongly that we use a
stationary Cartesian coordinate frame, x1, x2, x3,
to describe the geometry of the element and to work with
our element.
This coordinate frame, x1, x2, x3, is stationary.
In that stationary coordinate frame of course we are
measuring the coordinates of any material particle
corresponding to time 0, corresponding
to time t, et cetera.
The same way as we discussed it in earlier lectures when we
talked about the analysis of solids, 2-D and 3-D solids,
and when we talked about the continuum mechanics equations.
So here these coordinates of the material particles, as the
material particles are moving through the stationary
coordinate frame, are given by the right hand side.
And what do we see here?
k is 1 to n, n is the number of nodes for the element that
I've shown you and would be nine.
h k are the interpolation functions corresponding to the
two-dimensional surface of the element.
In other words, these h k's are really the 2-D
interpolation functions as we are used to see them for plane
stress, plane strain, and axisymmetric analysis.
Same interpolation functions.
These are the nodal point coordinates at time 0.
Here we have t, that is the third isoparametric
coordinate.
We talked about it just now.
k, going from 1 to n again.
a k are the thicknesses at the nodal points.
h k here is exactly the same h k that you see here.
And these are the direction cosines of
the director vectors.
Director vector n means director vector k, or normal.
n really stands for normal, but it's really the director
vector referring to the director vector k,
of course, a node.
0 means time 0 and i means the components, the three
components of the director vector.
That's what we're looking at here.
Now if you leave this term out then you would have simply the
interpolation of the mid-surface as for a membrane
element, of course curved mid-surface.
This term here is added in to take into account the effect
of the shell thickness.
Similarly at time t we have, applying the same
interpolation t, x, i here now.
Here we have t, x, i, k, same h k that we talked about
earlier, same summing that we talked about just now.
Here now t, v, n, i, k, the direction cosines, also
director vectors.
Director vector k at time t now.
Notice that all we have done in this term and in that term
is to substitute for the 0 that we had here and that we
had there, the t now.
Of course this t means time t, this t here
means coordinate t.
That's why we put a circle around it and wrote it out
there once more.
This is the coordinate, the isoparametric coordinate t.
r s coordinates go in here, t coordinate goes in there.
What has happened here is that originally our director vector
might look like shown in this picture here.
The node coordinates are given here, 0 x i k, and in the time
from time 0 to time t this director vector moves to look
as shown now here.
And of course the nodal point itself has moved as well.
So it's these quantities here, these [? rad ?] quantities
that we're using here, which carries a curve.
Well, to obtain the displacement of any material
particle within the shell we proceed now exactly the same
way as we have proceeded in the development
of 3-D solid elements.
We take the interpolation for the geometry at time t,
subtract the interpolation for the geometry at time 0 and we
get the displacements corresponding to time t.
The result is this equation here.
Here we have the displacements of any material
particle in the shell.
Here we have the nodal point displacements from
time 0 to time t.
Here we have the director vectors at time t, so to say,
minus the director vectors at time 0.
Really these are the direction cosines corresponding to the
director vector at time t, minus the direction cosines of
the director vector corresponding at time 0.
Of course this quantity here is obtained by this equation
and that quantity here is simply obtained by subtracting
the right hand sides corresponding to t x i and 0 x
i the way you just have seen them on the previous
viewgraphs.
The incremental displacement from time t to time t plus
delta t is similarly obtained from this relationship here.
And the result is shown here where now we have here the
increments in the nodal point displacements.
And here we have the increments in the direction
cosines of the director vectors from time t to time t
plus delta t.
The equation is given right there.
Well, with the equations that we have developed so far we
are almost ready to establish the strain displacement
matrices for the T.L. and U.L. formulations of the element.
We have the coordinate interpolations for the
material particles.
We discussed those.
And we have at the moment also the interpolation of the
incremental displacements of the material particles in the
shell element in terms of nodal point incremental
displacements and the increments of the direction
cosines of the director vectors at the nodal points.
What we, however, want is to have the incremental
displacements in terms of the nodal point displacements and
nodal point rotations.
The nodal point rotations because the incremental nodal
point displacements and nodal point rotations are the
engineering type quantities that we can nicely deal with
in a computer program when we analyze shell structures.
So what we want is to express v n i k, the increments in the
direction cosines of the director vectors, from time t
to time t plus delta t in terms of
the nodal point rotations.
And that is achieved as follows.
Here we have the stationary coordinate frame x1, x2, x3.
e 1 is a vector into the x1 direction, e 2 the vector into
the x2 direction, e 3 the vector into the x3 direction.
Here we show v n k for nodal point k.
In other words, a director vector, at time 0.
This one is input by the analyst.
These two are calculated in the program.
And of course there are such two for every nodal point k.
For every nodal point k we also put in a director vector.
Now the convention that is used, that can be used for the
v 1 and v 2 calculations, that convention is given down here.
Notice that if v n points into the e 3 direction then v 1
points into the 1 direction and v 2
points into the 2 direction.
By that I mean into the e 1 and into the e 2 directions.
Notice, this is a detail, that when v n points into the e 2
direction this formula breaks down and you need to use some
other convention.
But that is a detail.
We don't really need to discuss that
very much here now.
Anyways, let us say then at every nodal point k, v n has
been input by the user, v 1, v 2, calculated by
the computer program.
We notice that these two are once again
perpendicular to v n.
Then we can directly say that the increment in the direction
cosines of the vector, the director vector, is given via
this relationship here.
Now I've written this down already for time t.
Of course it also holds for time 0, all you do is
substitute for t, 0.
It holds in fact for any time of the motion that we are
considering.
Let's see why this holds.
Well, this picture here shows what's happening.
Here we have v n, here we have v 2, here we have v 1.
Notice alpha is the rotation about v 1, beta is the
rotation about v 2.
Notice that with the rotation beta about v 2 here, we of
course have an increment in this vector shown by this
component because this here is now v n at time t plus delta t
when alpha k is 0.
When alpha k is 0.
Now of course you would also have the alpha k component
coming in and that means you have to add also this term.
Notice that once you have obtained this vector you want
to normalize its lengths again.
But this picture here shows why this term is a correct
term to use in this formula and you can extend this
picture to also include this term.
With this relationship we can substitute for v n and that's
now done in this equation.
We have substituted for v n and have now our increments in
the displacements for the material particle within the
shell in terms of nodal point incremental displacements and
rotations about these v 1 and v 2 axes that we defined.
Well, having established this interpolation for the
incremental displacements and, of course, the interpolations
for the geometries of the element at time 0, at time t,
we can directly establish the strain displacement matrices.
And we will see we can then set up the k matrix, the f
vector, the elements that go into the equilibrium equations
the way that we discussed it in the earlier lectures.
And from the solution of k u equals r or k delta u equals
delta r in nonlinear analysis, we of course get our nodal
point rotations, alpha k and beta k.
And once we have calculated these nodal point rotations we
obtain by this relationship here the v n at time
t plus delta t.
In other words, what we're doing really here is we
integrate over all of the angle, alpha k and beta k, to
get a more accurate approximation for the nodal
point vector, of the director vector, I should say, at time
t plus delta t.
Notice that if you do this integration in one step with
the Euler forward method, you get back the equation that we
had earlier on the viewgraph.
And which I tried to explain or discuss with you using this
picture that you saw.
And I mentioned also that after this integration of
course we want to normalize the lengths of this vector to
make it always a unit length vector.
We recognize that with this approach we have only five
degrees of freedom per node.
Three translations in the Cartesian coordinate
directions which are stationary, and two rotations
refer to the local nodal point vectors v 1 and v 2 at time t.
Now notice in geometric nonlinear analysis, of course,
this vector and that vector, t v 1 and t v 2, change
direction so our alpha k and beta k are rotations that are
measured about changing directions.
That is an important point to recognize.
Let's look at one pictorial
representation of what's happening.
Here we have node k.
We have a smooth shell, say, that is discretized using four
shell elements.
I've taken one shell element away as shown here so that we
can look into the shell.
And at that node we have, as shown now, v 1 and v 2 at time
t and the director vector corresponding to a time t.
We measure at that time alpha k and beta k
about v 1 and v 2.
And we also measure the displacements of the node, u
1, u 2, u 3.
So notice that this node moves as shown.
These are the three translational degrees of
freedom and this director vector here moves to a new
position and also changes direction.
And that new director vector of course is
given here in red.
Notice that there is no physical stiffness
corresponding to the rotation about the director vector.
No physical stiffness.
The five degrees of freedom that the element very
naturally carries, u 1, u 2, u 3, alpha k, beta k.
Alpha, beta at every node k.
If only shell elements connect to node k and the node k is
not subjected to boundary-prescribed rotations
then we only need to assign these five degrees of freedom
to the node and only work with these five degrees of freedom
at that node.
However if we deal with a node to which also beam element is
connected, which of course in general has three rotational
degrees of freedom, or a node on which a boundary rotation
other than alpha k or beta k is imposed then we transform
the two nodal rotations, alpha k and beta k, to the three
Cartesian axes.
Because this way we can directly deal then with the
connection here and the imposition of
the boundary rotation.
We can do so directly using these three rotations now
measured in the Cartesian axis directions.
I mentioned already that the above interpolations for 0 x
i, t x i and u i, in other words, for the original
geometry, the current geometry, and the incremental
displacements the way we have developed them, they can
directly be used to obtain the strain displacement
transformation matrices.
And we really do so in the same way as for the 3-D solid
elements which we discussed in an earlier lecture.
However, there's one method to recognize, and I briefly
pointed it out also already in the earlier lecture, that
using this expression here--
and I now must refer to the earlier material that we
discussed--
using this expression to obtain the strain displacement
matrix, we realize that we obtain the exact linear strain
displacement matrix.
However, using this expression here to develop the nonlinear
strain displacement matrix, t 0 b n l, for the shell element
only in approximation to the exact second-order strain
displacement rotation expression is obtained because
the internal element displacements depend
nonlinearly on the nodal point rotations.
I pointed that out earlier.
Please refer back to that discussion to obtain a deeper
understanding of what I mean here.
The important point, of course, is that we do obtain
the exact linear strain displacement matrix, so at
convergence in an iteration, k delta u equals delta r, when
we have converged we actually have the exact solution to the
model that we're using, of course.
So this is important that we obtain the appropriate and
exact t 0 b l matrix.
The effect of what we are neglecting here was earlier
mentioned and please refer back to that lecture.
We finally need to still impose the condition that the
stress in the direction normal to the shell
mid-surface is zero.
Remember this was one further assumption that we discussed
at the beginning of this lecture.
We use a direction of the director
vector as a normal direction.
This means that at each Gauss integration point within the
element, and which we want to evaluate the stress-strain
law, we first of all set up a system of vectors, e bar r, e
bar s, e t, that are mutually perpendicular.
Now let's look here into the picture above and we see here
at a particular Gauss point, schematically shown, the
vector e r and e s which are vectors corresponding to the r
and s axes.
e t is a vector corresponding to the direction of the
director vector at that point.
e t we accept as the normal direction, that's for the
shell at that point, and we construct e bar s and e bar r
to be vectors perpendicular to e t and to themselves.
And that is achieved by this relationship here.
Having now established e t, e bar r and e bar s, we use this
stress-strain law.
And by this I mean let's look first what's
in these round brackets.
We use this stress-strain law corresponding to these
directions.
In other words, the directions e bar r, e bar s and e t where
this is the normal direction, this corresponds to the normal
direction e t.
Notice by putting zeroes here we impose the fact that into
the direction e t we have zero stress.
Of course this matrix is symmetric.
Notice we have k here which is a shear correction factor
applied to the transfer shear stresses in the shell.
New of course is Poisson's ratio and
e is Young's modulus.
Now this is the material law corresponding to e t, e
bar r, e bar s.
And what we now have to do is transform this material law at
every integration point to the global directions.
Global directions because for the global x1, x2, x3
directions we have established the b, the strain
displacement matrices.
And that gives us this material, or c, shell.
This q s h t, q s h is, I think, quite well known.
Let me show you the form of it briefly.
It's a transformation matrix where we show some of the
terms here, as you can see.
And these terms, l 1, m 1, n 1, et cetera, are
defined down here.
And l 1, for example, is nothing else but the cosine of
the angle between e 1 and e bar r.
In other words, it's a transformation matrix that you
are probably quite familiar with in linear analysis.
It's the matrix that transforms the stress and
strain components from one coordinate system to the other
coordinate system.
And of course the coordinate systems that we are
transforming, that we're using here, are the bar, e bar, r, e
bar s, e t coordinate system on the one side and e 1, e 2,
e 3 on the other side.
Well, using this matrix we assure that the columns and
rows 1 to 3 in c s h reflect that the stress normal to the
shell mid-surface is zero.
This holds true because, remember if we go back once
more to the viewgraph, we have set this column and
corresponding row to zero elements.
And of course this means that the stress normal to the shell
surface is zero.
I should also briefly point out that we have a plane
stress condition corresponding to the other direction of
stresses, in other words, the e bar r and e
bar s direction stresses.
We have a plane stress condition as you can see here.
And of course this term would go with it as well.
This term and these terms here reflect the plane stress
situation in the plane of the shell, zero
stress through the thickness.
And all that we are transforming to the global
system now here--
that fact, that physical fact--
of course must still be reflected in c s h.
And that's what's being said here at that point.
If you want to do plastic analysis, creep analysis, you
proceed in the same way.
But you calculate then once again the stress-strain
metrics as in the analysis of 3-D solids.
And having got that stress-strain matrix, six by
six matrix, you impose the condition that the stress
normal to the mid-surface is zero in much the same way as
what we have done here for the elastic material condition.
Finally, regarding the kinematic descriptions that we
talked about for the shell elements, it is interesting to
note that also transition elements can be developed.
These can be quite useful in practical analysis because
they are elements with some mid-surface nodes that carry,
in other words, associate director vectors and five
degrees of freedom per node and some top and bottom
surface nodes with three translational degrees of
freedom per node.
These elements would be used, for example, to model
shell-to-solid transitions or to model shell intersections.
And here you see one such typical element just
schematically shown.
Here we have a mid-surface node, three translational
degrees of freedom corresponding to the
stationary coordinate frame, two rotational degrees of
freedom the way we talked about it just now, mid-surface
node here and top and bottom nodes here with three
translational degrees of freedom for
each of these nodes.
Notice we can directly couple 3-D solids to this phase here
and shell elements to this phase here.
We haven't shown mid-surface nodes here, but you would,
say, have all the mid-surface nodes here and then surely
shell element can directly be coupled into here in such
situation as schematically shown right down here on this
viewgraph where we have solid elements on this side and
transition element right there and shell
elements on that side.
Because here you would continue with shell elements,
you would continue with solid elements here.
And once again three translational degrees of
freedom for these top and bottom surface nodes and five
degrees of freedom at shell mid-surface nodes as shown for
that node right here.
Notice we can also use these transition elements to model
shell intersections very nicely as exemplified up here.
Well, this brings me to the end of what I wanted to
discuss with you in this lecture.
Of course what we have not done yet is to look at example
solutions and what I'd like to do in the next lecture is
first of all talk with you about beam elements, the
isoparametric beam element, which is formulated much in
the same way as the shell elements
that we just discussed.
And then I'd like to show you applications of the beam
elements as well as the shell elements.
So please, if you are interested in this subject
matter, continue looking at the second tape, part two of
this set of lectures.
Thank you very much for your attention.