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 would like to continue to consider the
plate with a hole that we already considered in the
previous lecture.
But I now would like to turn our attention
to a nonlinear solution.
As we mentioned in previous lectures, a nonlinear analysis
should only be performed only once a linear solution has
been obtained.
The linear solution checks the finite element model and
yields valuable insight into what
nonlinearities are important.
And once again, we considered the linear solution of this
plate in the previous lecture.
We now want to go on with the nonlinear solution.
Here we have the plate with the hole once again.
It's a square plate subjected to the loading shown.
Here is the whole.
These were the material data that we used
in the linear analysis.
The thickness of the plate is given here.
We consider only one quarter of the plate because of
symmetry conditions, we can considering that one quarter,
analyze the whole plate, as we have discussed in
the previous lecture.
In the previous lecture, we also showed how we use
ADINA-IN to generate the data for this mesh.
And this input data then is used in ADINA to actually
perform the analysis.
We did the analysis for linear conditions in
the previous lecture.
Some important considerations for the nonlinear analysis are
now what material model to select, what displacement
strain assumptions to make, what sequence of load
application to choose, and what nonlinear equation
solution strategy and
convergence criteria to select.
We will address these issues in this lecture.
We use, once again, the ADINA system.
Now, of course, for the
elasto-plastic static response.
We will also investigate the effect on the response when a
shaft is placed into the plate hole.
Some important observations regarding the nonlinear
analysis are given on this viewgraph.
First of all, we notice that the recommendations that we
discussed regarding the linear analysis that we discussed in
the previous lecture are also very valid here of course.
But for the nonlinear analysis, we need also to
consider and be careful with the sequence and incremental
magnitudes of load application and the choice of convergence
tolerances.
We ill address, of course, these issues just now.
The first analysis that I'd like to discuss with you is a
limit load calculation of the plate.
Here we show the plate and the load, p, will increase
continuously up to a maximum value and then decrease to 0.
The plate is modelled as an elasto-plastic material.
And the material assumption is summarized on
this viewgraph here.
Here are the material properties.
We assume basically it is a steel.
Notice the stress strain law is shown here.
We assume isotropic hardening in the analysis.
We discussed what this means in an earlier lecture.
The initial Young's modulus is the one that we use for the
linear analysis.
Nu is equal to 0.3.
And the strain hardening modulus is given here.
This idealization is probably only applicable to small
strain conditions, strains that are
smaller than 2% roughly.
The maximum that you would want to allow is probably 4%.
And we will actually perform the analysis first using a
materially nonlinear only formulation.
This means, as we discussed in the early lectures, that we
neglect all kinematic nonlinearities, that we only
include the material nonlinearities in the
analysis, these material nonlinearities.
Later on, we however want to also perform in this lecture
an analysis that includes the displacement large quotations
and in fact even large strain conditions.
And we will study those analysis results in comparison
to the material nonlinear only analysis results.
The load history used for the analysis is
shown on this viewgraph.
You can see that we are increasingly linearly the load
up to a maximum value of 650 MPa, megapascals, and then
suddenly decrease the load to 0.
Notice we are using altogether 14 steps, 13 to increase the
load and just one step to decrease the load.
Of course, we are having here a time axis.
But the load step or time step that we used was
delta t equal to 1.
Well we performed this analysis a few weeks ago in my
laboratory at MIT.
And we brought in a video crew to video record our actions.
I'd like to now share with you what we have recorded and also
narrate to you what actually is happening in the computer
run as we prepare the computer run, as we run it, and also
interprets the resides.
Our first step is to modify the input data that we
prepared in the previous lecture for the linear
analysis of the plate.
We now have to, of course, modify this input data.
First of all, to introduce the load curve, this load history
curve that we just discussed.
And then we also have to modify the material data to
correspond to the elasto-plastic material data
that we now want to associate with a plate.
So let us look now at the video record of what we did
some weeks ago in my laboratory at MIT regarding
the change of these input data.
Here we see once more the mesh that we're using
to analyze the plate.
And now we prepare input data for ADINA-IN.
Here we input the time function that we employ.
You recognize the function points for time 0, 13, and 14
with the values 0, 6.5, 0.
We also input that 14 steps are used in the analysis, that
time step delta t is 1.
Next we input the material definition.
And note that there is a typographical error.
We typed plestic instead of plastic.
We try to do the typing fast and did not notice the error.
Notice the Young's module E, Poisson's ratio nu, the strain
hardening modulus ET, and the yield stress [? sigma ?]
yield are defined.
Because of the typographical error, the program prints out
an error message, namely the plestic material is not found
in the library.
Here we see the library of material models
available in ADINA.
The library consists of the material models elastic,
orthotropic, thermo-elastic, and so on and so on.
We know retype the material data definition.
We also do not want to use equilibrium iterations.
The default in ADINA is to use equilibrium iterations.
Actually, the BFGS method we discussed earlier because
large errors of solution can accumulate when
iterations are not used.
We discussed all of this earlier.
Let's see what happens when we do not iterate in the solution
of this problem, just as a point of study.
We now finally by the command ADINA generate
the ADINA data input.
Note that in this input preparation we only change the
data from the linear analysis data used in the previous
lecture to the data for the nonlinear analysis we want to
perform now.
Having set up the proper input data for ADINA-IN and having
used ADINA-IN to generate the input data for ADINA, we can
now execute that input data with ADINA obtain our first
analysis results.
We evaluate these analysis results by plotting the force
applied here as a function of the displacements
corresponding to this motion as well.
And we will see that the force displacement curve looks
rather unphysical.
In other words, the results don't make
much physical sense.
So we search for an explanation.
Why is that so?
And we will find that the reason is that we did not use
equilibrium iterations in the analysis.
In fact, if you go back, you will see that we deliberately
did not want to use equilibrium iterations in this
first analysis, although in ADINA the default is to use
equipment directions.
But I wanted to once show you what kind of results you must
expect if you don't use equilibrium iterations.
So we realized that we should really use equilibrium
iterations and that we will, of course, have to change our
input a little bit through ADINA-IN in order to perform
equilibrium iterations.
The load history that we will still be using is the same.
Here it is shown once again.
But now we will use the default method of equilibrium
iterations, the BFGS method.
And this one will be applied, this method of equilibrium
iteration will be used for each load step.
Once again, 13 load steps up and one load step down.
The convergence criteria that we using in the analysis are
show here, the convergence criteria on energy.
And we talked about this one quite extensively in a
previous lecture.
And the convergence criteria on the force, again, I'd like
to refer you to our previous lecture.
When we apply equilibrium iterations in each step, we
will see that our results look good.
They make physical sense.
In fact, they look quite appealing.
So let us look now at these solution results.
Let us go, in other words, to what has happened in the
laboratory the way we have been video
recording it earlier.
Here we see the solution results, the load applied as a
function of the displacement, the extension
of the quarter plate.
On the horizontal axis, we measure the displacement.
On the vertical axis, we measures of value of the load,
actually the pressure applied.
So far the curve looks OK.
But we show here only the responsible for the first 13
steps for which the load has increased monotonically.
here we see now the load displacement
response for all 14 steps.
Notice that the scale on the horizontal axis measuring
displacement is different from what we used before.
Note that the 13 first steps bring us to the maximum load
and maximum positive displacement and that the
predicted unloading response in step 14 is quite
unrealistic.
We obtain a large negative displacement.
As we will see, this is due to not having used equilibrium
iterations.
Next, we look at the mesh and study the plastic zones as
they develop with increasing load.
A time code is given about the mesh.
This time code gives the step number.
It increases until time is equal to 14.
The plastic zones are shown by shading the
area that is plastic.
For the first steps, there's no plasticity.
Then the plastic zone is small, it develops around the
hole and it grows rapidly as the larger
load levels are reached.
Note also how the plastic zone spreads through the elements.
We used 3 by 3 Gauss numerical integration and test whether
an integration point has gone plastic.
If so, we shade the contributory area of the
integration point.
As an average for each integration point, the
contributory area is 1/9 ninth of the element area.
Here at step 12, you can very nicely see how the plastic
zones have progressed through the elements.
The elastic plastic interface boundary
goes through the elements.
Note that at step 14, after unloading much off the plate
is still plastic.
This is quite unphysical.
We now rerun the analysis with equilibrium iterations and
here is the load displacement response we now obtain.
First we look at the scales on the axes.
We note that the loading response is similar to what we
had before.
Although a much larger displacement is
reached in steps 13.
The unloading response in step 14 is now quite realistic,
with a permanent positive displacement at zero load.
Finally, we show the plastic zones for this analysis.
Note that we show the initial mesh time 0 and then
immediately the time equals 6 results.
Initially, the plasticity progresses as much as in the
analysis without equilibrium iterations, but the final
spread of plasticity reached in step 13 is larger.
And after unloading of the load at the end of the
analysis, the complete plate is elastic.
However, clearly permanent deformations have occurred as
can be seen by looking at the default mesh at time 14.
As we discussed already, our analysis results now look
quite good.
They look quite reasonable.
But one additional way to evaluate the analysis results
is to plot stress vectors.
We did so in the linear analysis of the previous
lecture when we also looked at the analysis results obtained
from this mesh, but of course, in linear analysis.
We want to do now the same for the nonlinear analysis results
that we obtained.
And let us just quickly look at what we're doing in the
stress vector output.
We plot at each integration point two lines as shown here.
If they are carrying an arrow, then it is tensile stress.
No arrow means compressive stress.
And notice these two lines correspond to
the principal stresses.
Notice that the lengths of these lines are proportional
to the magnitudes of the stresses.
So let's now do a stress vector plot for the mesh at
time 13 and at time 14, in other words, at maximum load
application and after removal of the total load, four the
results that we just have obtained.
Here we see the stress vectors plotted onto the total mesh
for the stress state at time 13, that is at total load.
We note of course, that there is very much information,
there are many stress vectors.
To see any detail we have to focus our attention onto
certain elements.
Here we now look closer at the elements adjacent to the
horizontal symmetry line.
We note that the stress vectors correspond to vertical
tensile stresses as expected.
At a top edge of the plate we see tensile vertical stresses
and tensile horizontal stresses.
The maximum stress at any integration point is 1100
megapascals and occurs near the hole.
Here we now see the stress vector plot at time 14, that
is after load removal.
It is most interesting to study the
stress flow in the mesh.
Note that the stresses flow along and parallel to the free
surface of the plate.
This must be so because there are no externally applied
tractions anymore.
Here we see the detail of the stress flow in the
corner of the plate.
The stress vectors are parallel to the free surface.
And here is the stress flow in the elements around the hole.
The same observations apply.
The maximum stress is 880.3 megapascals.
This completes what I wanted to show you in this phase of
the analysis.
This completes our materially nonlinear only
analysis of the plate.
However, if we look at the solution results once more
closely, we find that in this element here the magnitude of
the strains is about 2% at the end of load step 11, 4% at the
end of load step 12, and 14% to 15% at the end
of load step 13.
In other words, at maximum load application, we have
certainly here large strains.
And one might very well ask, what is the effect of this
large strain on the analysis results?
Of course, in the materially nonlinear only solution, we
did not include any kinematic nonlinearities.
So our next objective is then to perform analysis that said
include kinematic nonlinearities.
And we want to now proceed with a total Lagrangian
formulation analysis, which includes large displacements,
large rotations, but only small strains.
And I also want to share with you some solution results that
we obtained using an updated Lagrangian formulation.
We did not talk about this formulation
in the earlier lectures.
We did talk about this formulation, but not about
that formulation.
This formulation really is best covered
in a separate lecture.
However, it's still very interesting to look at the
solution results that we obtain we this formulation.
If you want to read up on this formulation, please refer to
the study guide in which a reference given.
A paper is referred to in which this
formulation is described.
So let us now look at the solution results obtained from
these three formulations.
And the solution results that we want to look at are once
again the force displacement curve for each of these
formulations.
In other words, force applies here, displacement seen here,
for these three formulations.
Let's turn back to the laboratory and see what are
the results.
Here we see the analysis results for the MNO, that is
the materially nonlinear only, the TL, that is the total
Lagrangian, and to UL, that is the updated Lagrangian
formulations.
We look first at the horizontal axis scale giving
the displacement.
And then at the vertical axis scale giving the load that is
the pressure applied.
Notice that there are three, in fact we will we later four
distinct curves.
However, under this much plasticity, the curves are
almost the same.
The TL analysis results corresponds to the smallest
displacements.
The MNO solution gives larger displacements.
And the UL solution gives the largest displacements.
For the UL solution, we actually see two curves when
looking closely.
These correspond to using once 14 steps as for the TL and MNO
analyses and then using once twice the
number of load steps.
Note that the unloading response in all solutions is
quite the same.
However, of course, the permanent displacements at 0
applied load are quite different because the maximum
displacements corresponding to peak load were different.
These analysis results underline the importance of
choosing the appropriate kinematic
formation for the analysis.
Here, large strain effects are quite significant at the very
high load levels.
In the next analysis we now consider the effect of a shaft
in the hole.
Notice, we look at the same plate as before except that we
know first consider elastic condition only.
And the shaft is shown here.
The shaft has this Young's modulus and Poisson ratio,
same as the plate.
But it is 5 times thicker than the plate and for the shaft we
also consider plane strength conditions.
What we want to do is place a shaft in there, the shaft
being initially flush with the hole, assuming no friction
between the shaft and the hole.
And then we pull on the plate and want to investigate what
is the effect of having that shaft there.
The analysis input data have to now be modified because we
have to put the shaft in there using finite elements as shown
here in red.
We used collapsed 8-node elements to
represent the shaft.
In other words, these collapsed 8-node isoparametric
elements become, of course, triangular
elements as shown here.
Notice we now have a contact surface here.
And that contact surface is modeled using a contact
algorithm, which we did not talk about in
this series of lectures.
This again, would be best covered in another lecture.
I'd like to refer you here to another paper, the reference
of which is also given in the study guide, if you're
interested in reading about the contact algorithm.
The contact algorithm can take into account friction
conditions as well, but in this particular analysis, we
assume 0 friction along the contact surface.
The solution procedure that we are using is it the full
Newton method without line searches.
And the convergence criteria that we are
using are listed here.
These we have been talking about earlier already.
Here we now because of the contact conditions have to
introduce also this convergence criterion, which
is really a convergence criterion on the incremental
contact force.
So let us now proceed with this analysis.
And once again, we perform the analysis and of course, we're
looking at solution results.
Here we see the mesh of the plate once more, the mesh we
used in the previous analyses.
We now need to change the input data for the analysis to
also define the shaft.
This is done using ADINA-IN.
We need to define the addition nodal points and elements for
the shaft in the same way as we input earlier the nodal
points and elements of the plate.
Let's look at the information that defines the content
condition between the plate and the shaft.
And here we see the input for ADINA-IN.
There are two contact surfaces.
The one is the plate hole surface and the other is the
shaft surface.
We denote these two to be a contact surface pair.
Here you now see the mesh of the shaft and the plate.
The shaft is defined by triangular elements.
Here we see the default mesh at maximum load.
Note that the plate has been extended vertically and has
shrunk horizontally.
The shaft has prevented the hole to shrink much
horizontally.
And on top off the shaft, a gap has opened.
All of these deformations are quite realistic.
Here, we see just the shaft and the ring of elements of
the plate around it.
Once again, the calculated deformations make sense.
If you look closely at the shaft by itself, you observe
that it has been compressed horizontally by the plate.
Let's look next at some stress vector plots.
These also show that a physically realistic solution
has been obtained.
Here we see the stress vectors in the element layer of the
plate around the shaft.
Note that the stress vectors are plotted onto
the original mesh.
For the element adjacent to the horizontal symmetry axis
off the plate, we see a vertical tensile stress and a
horizontal compressive stress.
Such stresses are to be expected.
The horizontal compressive stress is, of course, due to
the contact with the shaft.
Note that going around the shaft, the stresses in the
plate align to be parallel to the free surface of the hole,
since there is only contact near the horizontal symmetry
axis of the plate.
This completes what I wanted to discuss with you for this
phase of the analysis.
Finally, I would like to look with you at the analysis
results we obtained when we apply to this plate with the
shaft 100 MPa up there and down here.
We assume that they plate is made of an
elasto-plastic material.
In fact, we model that material as shown
in our early analysis.
And in addition to this loading here shown, also the
shaft expands.
It expands uniformly.
And in fact, it expands 0.05% based on the initial
dimensions of the shaft during each load step and we apply 10
load steps.
So the loading then all together is in the first load
step, 100 MPa applied here.
And from the second to 11th load step, we expand the shaft
by 0.05% in diameter, so to say, based on the initial
dimensions.
We use the updated Lagrangian formulation to model the
response of the plate.
Let's look now at these analysis results.
Here we see just as a reminder once more
the mesh we are using.
Also, here is once more the detail of the
mesh around the shaft.
This is the default mesh at step 1.
The deformations are due to the tensile load of the 100
megapascals on the plate.
Next we plot the plastic zones in the plate as they develop
when the shaft expands.
Notice again the time code above the mesh giving the step
number since delta t equals 1.
There are all together 11 steps.
The shaft expands from step 2 step to step 11.
We see the time code running and at time 7 we see the first
plasticity.
This plasticity spreads as the shaft further expands.
The maximum plastic zone is, of course, reached at the
maximum expansion of the shaft, that is at time 11.
This completes what I wanted to say about this analysis.
Note that after each analysis step we looked at the
calculated deformations and stresses is to identify
whether these make sense.
This brings us to the end of this lecture and to the end of
this course.
I'd like to now just take a few minutes for some closing
remarks regarding the course.
I mentioned already in the first lecture that nonlinear
finite element analysis is a very large field.
There are continuum mechanics principles, numerical
algorithms, and software considerations.
We could not cover in detail many aspects of all of these
fields in these 22 lectures.
However, I do believe that the 22 lectures provide a good
introduction and a good foundation for further study.
I would hope that you would listen to these lectures with
your colleagues, that these lectures would initiate
discussions, stimulations for your work in nonlinear
analysis and, of course, also questions.
We at MIT continue to work in nonlinear
finite element analysis.
And we also offer from time to time weekly courses.
I would be glad to see some off you at these weekly
courses to share some of the experiences that you have had
listening to these video lectures and also regarding
your work in practice.
Finally, I'd like to mention that a video course of this
nature can only be produced through the concerted effort
of a number of very devoted people.
I'd like to thank for their collaboration and support Dick
Norris, Elizabeth DeRienzo, Pat [? Regan ?]
of the Center of Advanced Engineering Study at MIT, and
Ted Sussman, my student.
And very finally, thanks also for the crew around here.
Thank you for your attention.