Hello everyone, in this video from the Ansys How To series we will discuss
• what is multilinear hardening plasticity model?
• How to calculate its properties from the experimental data?
• and how to use it in Ansys Mechanical?
Let's go!
Here's a typical stress-strain curve for metals under uniaxial tension.
At the onset, they undergo linear elastic deformation where the stress developed in the material is directly
proportional to the strain, and the constant of proportionality or the slope of the curve
is the Young's Modulus of the material.
Once the stress developed in the material exceeds a limit, the response is no longer
linear, and this limit is known as the elastic limit.
Before the elastic limit is reached, upon unloading, the material can return to its original state.
If we further increase the applied load, the material starts developing plastic strain,
meaning that if the part is unloaded, there's permanent deformation developed in the material.
It is important to remember that the material continues to undergo some elastic deformation beyond this point.
The limit beyond which the material sustains plastic deformation
is nothing but its yield strength.
If we re-apply the load, the stress-strain response will follow the same path, but it'll
sustain new plastic deformation only after reaching the stress at which it was unloaded.
In other words, its yield strength has increased due to strain hardening.
Typically, metals follow a nonlinear response due to this hardening until necking develops
in the material.
Beyond this point, the stiffness of the material drops down and eventually fails at a stress
value which is nothing but its ultimate strength.
In Ansys Mechanical, we can model the strain hardening portion of the curve using either
a bilinear or a multilinear hardening model.
A bilinear hardening rule assumes a linear
strain hardening portion and is defined using a tangent stiffness which is nothing but slope
of this line.
A multilinear hardening model uses a piece-wise linear function to model the nonlinear strain
hardening response until the necking begins. So, it does not support the portion of the
curve with negative slope.
There are other material models available in Ansys Mechanical that can capture the damage
in the material but multilinear model can only capture the response up to onset of necking.
To define this behavior, we need to provide two sets of inputs:
Linear elastic behavior which is defined by the Young's modulus and Poisson's ratio
and Multilinear hardening which is defined by the plastic strain vs true stress where
the first data point indicates the onset of plastic deformation which is nothing but (0,
yield strength).
Now, one may ask why we go through the trouble
of inputting plastic strain vs stress instead of total strain vs stress.
This allows us to define both effects independently, which is useful if we have different temperature-dependent
data sets for elastic modulus compared with plastic strain vs. stress.
If we defined total strain vs. stress, we have redundant data point with elastic modulus
at yield, and we cannot resolve the difference if values are inconsistent?
Therefore, we separate material definition into elastic and plastic behavior.
The procedure for doing this straightforward with a few simple calculations.
I’ll show you how to do this with real experimental data.
Here’s the data for a 316L stainless steel sample.
The data is recorded from a uniaxial tension test.
This data is engineering stress and strain and it must be converted to true
stress and strain before we can separate it into elastic and plastic behaviors.
This is because the engineering stress and strains are calculated based on the dimensions
of the undeformed sample.
However, as the strain increases, the area of cross-section
of the sample reduces due to Poisson’s effect.
So, at higher strains the engineering stress
and strain deviates from the true stress and strain developed in the material.
This difference may not be significant in the deformation ranges that we’re interested
in but it’s always a good practice to properly define the material input.
The conversion from engineering stress and strain can be done using this set of equations.
where sigma_true and sigma_eng are true and
engineering stresses, and epsilon_true and epsilon_eng are true and engineering strains.
Note that these equations are derived assuming incompressible behavior.
For most practical cases, this assumption is not problematic but it’s worth keeping in mind.
Next, we must identify the point at which the material begins to yield.
An easy way of doing this is to identify the point at which the response starts deviating from linear behavior.
This can be done either visually, or for better accuracy, one may monitor the change in slope
of the curve and then identify the point at which the curve starts to deviate from linear behavior.
This point is nothing but the yield point.
One can use the same strategy to identify the point at which the material may be undergoing necking.
To do this, one may monitor the slope of the curve and check when it turns negative.
That indicates where damage within the material becomes pronounced, which is associated with necking.
Note that while there are damage models available in Ansys Mechanical, they
are outside of the scope of our present discussion.
Next, we calculate the slope of the curve up to the yield point which is nothing but
the elastic or Young’s modulus of the material.
The next step would be to calculate plastic strain.
This can be done by calculating the
elastic strain at that point and subtracting it from the total strain.
We do this at all the points in strain hardening region.
The elastic strain is calculated from the ratio of stress at a given point to the Young’s modulus.
This is then subtracted from the total strain at that point and what’s left
is the plastic strain.
A common mistake that users often make is to calculate elastic strain at the yield point
and subtract that constant value of strain from the total stress strain curve.
Elastic strain is not constant, it is increasing if the stress is increasing.
Our data is ready now. Let’s go back to the Engineering data and see how to define
linear elastic material properties as well as multilinear stress-strain data.
Open Engineering Data and make sure that units are set to system your data is measured in.
In the table of Engineering Data, define “New_Material”,
This only gives the name to the material that we will define next.
Now, we need to define material properties for the “New_Material”.
Insert Isotropic Elasticity from the toolbox
and define Young’s Modulus as calculated previously.
Poisson’s Ratio is another required material property for the linear elastic part of the material definition.
Next, insert Multilinear isotropic hardening to define plastic behavior.
Before copying the data, make sure that the units for stress match your data.
If everything looks good, go ahead and copy and paste the data.
Note that the first point in this table should be zero plastic strain and stress at yield point.
The stress-strain curve should be monotonically
increasing, so we must identify the region where it begins to dip down and discard that
portion of the data. In other words, negative slope of the plastic strain – stress curve
is not allowed in the standard plasticity models.
Now the material is completely defined, and we can run the example in Mechanical to show
how to apply the “New_Material” in the simple analysis.
In this this example, we will simulate tensile test on a dog-bone sample.
The first step is to assign “New_Material” to the geometry.
Under Geometry click on the
part and define Material assignment as “New_Material”
Since this is a nonlinear analysis due to metal plasticity,
we should turn on large deformation and Auto-time stepping under Analysis
settings and set initial substeps to 30, minimum substeps to 30 and maximum substeps to 1000.
This way we can apply the load gradually and capture the elastic and plastic deformation
of the material more accurately.
Next, we will apply boundary conditions, on one end the specimen is held at rest by
the fixture, so a fixed support is applied. On the other end of the specimen a displacement
of 17.78 mm is applied.
Now the model is set for solution.
Let’s hit the solve button.
Let’s plot the normal stress in Y and scope it to the named selection.
Next, let’s plot the total normal strain in Y direction at this node.
To do this, we will use
a user-defined result to plot.
You can review the available options when you’re
on Solution and change to Worksheet view.
We’re interested in plotting the total plastic
strain in Y direction. Select it, right click and insert a user-defined result.
While we’re here, let’s also insert an object to plot the total elastic and total plastic
strains in Y direction.
Next, select all of them, and change the scoping to the nodal named selection.
Let’s define one final item before we evaluate these results.
Insert a new user-defined result
and in the expression add epely+epply.
By doing so, we’re summing up the total elastic
and plastic strains.
So, based on our discussion earlier, these quantities should add up to
the total strain.
Let’s evaluate these results and see if that’s what we will get.
As you can see, they correlate very well!
So, we can see that in the elastic region
the total strain is equal to the total elastic strain but once plasticity sets in it is the
summation of both elastic and plastic strains.
Also, note that the elastic strain continues
to grow during plastic deformation as well.
Finally, let’s plot the normal stress as well as total normal strain at a node location.
Select these two objects and insert a chart feature.
Change the X axis to maximum total strain
and Y axis to maximum normal stress in Y.
Now let’s plot this data against the experimental data.
we used.
The simulated data correlates very well with
the data we prepared for the input into Engineering Data.
This serves as a verification to our input.
Before we proceed to conclude the video, let’s have a short important discussion.
The data that we input is discrete, so how does Ansys handle calculations where we don’t
have the data defined?
Ansys uses linear interpolation for all calculations within the range of the data defined.
If the strain in the material exceeds the maximum plastic strain defined, then Ansys does not extrapolate
but it continues to use the last data point.
In other words, the material behaves as perfectly
plastic material beyond this point.
So, the user must exercise caution to check if the
maximum plastic strain in the model exceeds this value, both in verifying the results
or if the model runs into convergence or element distortion issues.
In conclusion, the multilinear hardening plasticity model in Ansys is defined using plastic strain
vs true stress data.
We extract this information from experimental data by
• first converting it to true stress and true strain
• then identifying the point at which the material begins to yield.
• Once we do this we can calculate the elastic properties of the curve using the elastic portion.
• We can then calculate the elastic strain
developed in the material and subtract it from total strain to calculate the plastic strain.
• This is then input into Ansys Mechanical
to finish the material definition.
• Remember that the first data point should be (0, yield strength).
I hope that you have found this discussion useful.
If you liked this video, then please like share and comment.
Also, do subscribe to this
channel to receive updates and visit ansys.com/courses to discover more useful content.