Introduction

Material models that provide accurate simulation results matching experimental data are foundational to successful FEA simulation of real-world applications. Calibration of a material model to experimental data is an optimization problem where the "distance" between simulation and truth signals is minimized, indicating how "close" the model fits experiment. In this example, we will perform an overview of an example calibration, completing the spring-steel model calibration example model from Ansys Help using Ansys optiSLang and Mechanical from within Workbench. Please refer to optiSLang documentation for details about aspects of the process that we skip for purposes of brevity.

Material Model

The material model that will be used to "match" the experimental data is a nonlinear isotropic hardening model have a Voce hardening law given by the equation

where the unknown material parameters are

with resulting stress-strain curve

In Ansys Workbench Engineering Data, we parametrize the according material model parameters as shown here:

Test Specimen and Experimental Data

The test specimen and experimental force-displacement curve (truth) are displayed below:

The experimental data will be stored as a text file named force_displacement_ref.txt in the Workbench model user_files folder from where it will be referenced by optiSLang throughout the optimization process. A snippet of the file is shown below, noting that the Reference keyword is important for distinguishing these data from the simulation results:

Finite Element Model

The finite element model consists of the thin body tensile specimen mesh with solid elements, subject to an end displacement with the other end fixed, thus simulating a standard tension test. The mesh and applied boundary conditions are shown here:

The resulting force and displacement of the gauge section is written to a file called force_displacement_sim.txt for each run via an APDL command snippet. The format of the force_displacement_sim.txt file is identical to the force_displacement_ref.txt file with the exception that the word "Reference" is replaced with "Simulation", which allows optiSLang to differentiate between the two data sets. Additionally, an image of the plastic strain field is written to file.

Workbench Project

The final Workbench project schematic that we will develop is

Data Send

The Data Send component is used to manage which data is copied and saved for each Design Point run. By carefully selecting which files to save for each run, the project size can remain relatively small, thus it is not recommended to select large files, such as, results files, otherwise the project size can become prohibitively large. The following shows that we only need the following files to be saved for each run:

Signal Processing

The Signal Processing component is where all aspects of data handling and computations are defined. The following tabs in the Signal Processing wizard are explained in the following sections.

ETK

Here we define how the force_displacement_ref.txt and force_displacement_sim.txt files are handled. The setup for these files is shown in the following images, noting that the details are explained in optiSLang help documentation:

force_displacement_ref.txt

force_displacement_sim.txt

Files

The setup of the Files tab is shown here:

Variables

The Variables tab is where data and variables resulting from computations on data are defined. The layout of the Variables tab for this example is shown here, where variables are designated as responses by clicking on Add Variable, highlighted in yellow:

Reiterating that the goal for this example is to calibrate the signal from the simulation response to the reference signal, we need to define several signal conditioning and signal comparison operations. The following steps are defined, resulting in variables and/or responses - note that variables that are designated as responses are highlighted in green:

Create a variable for the reference displacement that will be used to interpolate the simulation signal based on the reference signal: disp_ref.
Interpolate the simulation signal using disp_ref so that both the reference and simulation signals have the same length. The resulting signal is stored as the Signal_interpolate response variable.
Compute the gradient of Signal_interpolate (Signal_interpolate_gradient) and its minimum (min_gradient_Signal) that will be used to ensure that the resulting signal has a positive minimum gradient, i.e., the slope at the end of the curve.
Create a linearly spaced displacement vector (disp_steps) that will be used to align the reference and simulation signals using fewer points at the same ordinates (displacement).
Extract the reference and simulation force values, at displacements defined by disp_steps, resulting in force_steps_ref and force_steps_sim responses, respectively.
Define a "distance" between signals by computing the root squared error between the force_step_refs and force_steps_sim signals, resulting in the RSE_signal response, which is to be the optimization variable that will be minimized.

Run Options

Run options setting defaults are used in this example. However, depending on licensing, parallel simulations may be conducted to reduce time to results.

Parameter Set

The final parameter table is shown here, noting that two additional parameters for plastic strain are added from the Static Structural analysis:

Adaptive Metamodel of Optimal Prognosis (AMOP)

A metamodel, also known as response surface, is a statistical model that relates the response to the inputs, generated by smart choice of the location of a small number of data points. The resulting surface is the mean of the response given the relatively sparse data. An adaptive metamodel enhances the standard metamodel by strategically adding input locations in order to minimize the variance in response prediction. Here, we utilize the AMOP as defined as follows.

Parameter

The input parameter values, types, and ranges are defined as shown here:

Start designs

This is blank since we are starting from scratch.

Criteria

Here, the optimization criteria are defined as shown in the Criteria pane below:

Adaption

We allow for a maximum of 150 design points to generate the AMOP:

MOP

For the definition of the MOP, we use most of the defaults, selecting the type of Tested metamodels as shown here:

Other

We leave the defaults in the Other tab.

Result Designs

This table, initially empty, shows the results of the design points. Note that some designs are considered infeasible as the minimum gradient constraint is violated in these (constraint column shown in the 2nd image).

AMOP Results

Here is a screenshot of some of the results that are available from an AMOP run:

If we focus on the Signal Plot in the top middle, we see that the "best design" (red trace) reasonably matches the reference signal (green trace). Furthermore, the Residual plot shows that the variance between the reference signal and AMOP predictions is small, thus indicating a good fit.

There are many more plots and diagnostics that one can use to determine goodness of fit. Refer to the optiSLang manual for more details.

Evolutionary Algorithm

The evolutionary algorithm is "nature inspired optimization" according to optiSLang. We use the top 10 best designs from the AMOP as start designs, making the optimization process more targeted and efficient. The Parameter settings are the same as for the AMOP, with the other settings detailed here below: