Metal plasticity is one of the most frequently
used material nonlinearity option available
in Ansys Mechanical.
It represents a wide variety of commonly available
ductile metals that are well understood to
yield in accordance with the Von-Mises Yield
Criteria.
When included in an FEA model, metal plasticity
may sometimes have a convergence challenge.
In this How To...video, we will explain how
to diagnose when a metal plasticity model
is a contributing factor in non-convergence.
Remember, when a ductile metal is loaded beyond
its elastic limit, covalent bonds, at the
microscopic level, begin to break and grain
boundaries begin to slip.
This phenomenon can be observed, at the macroscopic
level as “yielding” when non-recoverable
plastic strains and permanent deformation
begin to develop.
The effect of such yielding can also contribute
to a reduction of stiffness in the structure.
Such stiffness loss is a real physical phenomenon.
It is path dependent and it can be highly
nonlinear.
The common metal plasticity models available
in Ansys are Bilinear Isotropic, Multilinear
Isotropic, Bilinear Kinematic and Multilinear
Kinematic.
They are all programmed to predict yielding
in accordance with the Von-Mises Yield Criteria.
In this how to video, we will use a multilinear
plasticity model and show how to diagnose
convergence problems for metal plasticity.
First of all, about multilinear plasticity.
“Multilinear” allows users to represent
the stress vs plastic strain relationship
with multiple data points.
These data points can be directly input to
Ansys to define the plasticity model.
A very important thing to remember is, for
the multilinear option, elastic perfectly
plastic behavior is assumed for strains beyond
the last stress-strain data point entered.
Perfect plasticity, as shown here, can be
represented as a flat line, where plastic
strains will grow with no increase in stress.
To put it in other way, perfectly plastic
behavior represents a point of zero tangent
stiffness.
When an FEA model with metal plasticity fails
to converge, it is important to first understand
what the stress state of the material is at
the point of non-convergence.
In other words, where on the stress-strain
curve are we at a specific location.
Any amount of loading beyond the last multilinear
stress vs plastic strain data point can potentially
induce instability due to zero tangent stiffness
in one or more elements.
If this is occurring across an entire section
in a primary load path of the structure and
under a force-based load, this will result
in non-convergence.
If material is not on the elastic perfectly
plastic part of stress-strain curve, then
non-convergence might not be a physical instability.
It could be numerical instability caused by
very large load over one substep without ability
to recover via bisections.
Or perhaps an insufficiently constrained model
is causing a spike in strain energy in just
one nodal location.
Fortunately, the text in the solver output
helps to tell the story of the convergence
history from start to finish.
With a careful review of warnings, errors
and plastic strain development recorded in
the solver output, together with a careful
review of available stress and plastic strain
results, user can determine if nonlinear convergence
trouble is related to metal plasticity or
something else.
Let’s take a look at a simple example...
Here we are looking at a quarter-symmetry
model of a rectangular plate under a pressure
load.
Click on the geometry from outline tree, the
material assigned to it is multilinear structural
steel.
Let’s go to workbench and check the engineering
data for the material definition.
The definition of multilinear hardening is
defined here by table input.
Plasticity initiates when equivalent stress
reaches 260 Mega Pascal.
Note that, the strain input is plastic strain
instead of total strain.
Therefore, it starts from 0.
Also, we can see that the slope of the curve
decreases with each successive data point.
In Mechanical, we can review the definition
of the material when we click on “Material”
from the tree.
For the mesh, we applied a mesh size to the
thickness direction of the plate geometry
so that we have three layers of elements.
A pressure is added on one of the surfaces
of the geometry.
For boundary condition, we defined it to make
the geometry a quarter symmetric part.
In Analysis Settings, we switched on the auto
time stepping.
And defined initial number of substeps to
be 200, minimum substeps to be 25 and maximum
substeps to be 10000.
This means the solver will start solving the
problem with 200 substeps.
If everything goes well, it will try to gradually
increase the substep size, accordingly the
number of substeps will reduce, till the minimum
substeps defined as 25.
On the other hand, if the convergence is difficult,
the solver will gradually reduce the substep
size, resulting a greater number of substeps,
upto maximum substeps defined as 10000.
Another change we made under Analysis Settings
is that, we switched on the large deflection
formulation.
The reason we did this is,  with a plasticity material, we expect
geometric nonlinearity will kick in.
Before solving the problem.
Let’s go the Solution Information, put a
number 4 for Newton-Raphson Residuals and
Identify element violations.
The reason to do so will be explained later.
Now we are ready to test run the model.
For this problem, the solver runs for a certain
number of substeps and gets terminated.
You can see a yellow lightning bolt icon in the
Solution, indicating that the solution is
not completed.
Even though the simulation is not fully completed,
we can still check the results at those  converged
substeps to verify if the model is behaving
as expected.
Let’s have a look at the equivalent stress
and plastic strain results.
Click on the last converged point, which is
the one before the failure and click “retrieve
this result”.
We can see that most stress and distortion
is concentrated on the constrained edge.
A check of the plastic strain shows large
amount of plastic strain developing across
the section of the plate – in fact, the
amount of equivalent plastic strain exceeds
what we defined in our material input in Engineering
Data.
Checking the convergence history, it shows
that the last step is not converged.
Only when the purple point representing unbalanced
residual force is under the force criterion,
it’s a converged step.
You might wonder, could we check where the
unbalanced residual occurs on the geometry?
Here is when, the settings we put for solution
information come in handy.
By setting a number 4 for Newton-Raphson Residuals,
the solver will save the contour plot of residual
force for last 4 iterations.
The development of residual force can be visualized.
The area is evolving, and the amount of unbalanced
force drastically increases for the last two
iterations.
So what’s the problem then?
Why can’t the solver converge with so much
residual force?
Here, HDST shows the highly distorted elements,
and EPPL marks the elements with overly large
plastic increment.
The number 1 here means, it’s showing violated
elements for the last iteration, number 2
means second to the last.
For 1 iteration, there might be multiple groups
of violated elements.
Then the question comes, what if we allow
the solver to use even smaller substep size?
Will this problem converge?
If the maximum number of substeps were 10
or 100 or unspecified, then increasing the
maximum number of substeps can be beneficial.
But for this example, we have already set
the maximum number of substeps to 10,000,
so further increase will not help much.
Let’s pick a node in the critical region
and plot the stress vs plastic strain curve.
First of all, we need to evaluate the stress
and plastic strain respectively.
Now, click on the “Chart” from the Solution
tab, select the stress and plastic strain
for the node from Solution, set the X axis
as the plastic strain.
And put the labels for the two axes.
Now we are looking at the stress vs plastic
strain curve of the node.
We should neglect the last data point, as
it’s the last unconverged iteration.
What we observe here, is the curve is becoming
flat after this point.
The stress for this data point is about 550 Mega
Pascal and plastic strain is about 0.2.
This indicates that the points after this
point are beyond the multilinear plastic model
defined in engineering data.
As we mentioned before, such perfect plasticity
introduces instability to the system since
plastic strains can develop with no further
increase in the load.
Especially when there’s a group of elements
exhibiting perfectly plastic behavior at once,
we may see such non-convergence since a plastic
hinge has developed.
So, for this problem, how to overcome the
convergence?
In fact, in real life, it’s not normal to
see a material suddenly loose strength entirely.
When we define multilinear plasticity, the
material stress-strain data should be greater
than the expected strain range of the simulation.
In this case, let’s go back to the Engineering
Data, and add three more data points for the
multilinear plasticity.
Now, for the last data, stress is 730 Mega
Pascal and plastic strain is 0.95.
Let’s refresh the model and rerun the problem,
see if there any improvement.
You can see, with this change, this highly
nonlinear simulation solved successfully.
-
A quick summary for this how to video, when
included in an FEA model, metal plasticity
can sometimes be the source of a convergence
challenge.
When non-convergence is encountered in a structural
nonlinear application, it is important to
use different diagnostic tools in Mechanical
to understand the possible source of non-convergence.
Loading beyond the last stress vs plastic
strain data point, in a multilinear plasticity
model, can lead to non-convergence in a force-controlled
simulation, when the material yields through
a primary load path because of elastic perfectly
plastic assumption.
One way to overcome this is to add more stiffness
to the material by adding more points to the
stress vs plastic strain curve.
Ensuring that a sufficient number of maximum
substeps has been specified, will also allow
the solver to apply a smaller load increment
during a highly nonlinear portion of the load
history.
Reviewing the converged results, such as stress-strain
response at specific locations, as well as
checking the regions of element distortion
or high force residuals can also give you
a clue as to what kind of corrective action
is needed.
If you find this video helpful, please like,
comment, and subscribe.
To find more information about plasticity
or other topics, check our channel for more
how-to videos and visit ansys.com/courses
today!
