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!