About Material Calibration from Finite Element Simulation Models

Built-in Simulation Models Versus Imported FE Simulation Models

The built-in simulation models provide efficient and easy-to-use options for performing material calibrations, but they do have limitations that restrict their ranges of application. For example, the built-in models assume that the deformation in the test coupons is homogenous. This assumption precludes you from using the built-in models in some common testing scenarios, such as a uniaxial tension test in which necking occurs.

By creating and importing your own FE simulation models into the app, you can calibrate a material response using simulation models of arbitrary complexity. These models might include necking and failure or other general states of inhomogeneous deformation.

FE-based calibration requires a robust and run-ready model that provides a good engineering representation of the physical tests that you are simulating. Confirm that each FE model has the proper steps, time-dependent boundary conditions and loads, and response output locations (in the form of node and element sets) that correlate with the physical tests. For the error calculations, identify and match the response output requests manually to the proper columns of imported response test data.

In summary, the app defines the built-in material models completely during test data import, and they are ready for use in a calibration immediately. Imported FE models require a number of additional before you can use them to calibrate a material response.

Guidelines and Requirements for FE Simulation Models

An FE simulation model that is suitable for import in a calibration should be robust, efficient, and accurate. You can improve each of these qualities in a simulation using the following approaches:

• Robustness: During a calibration, the app samples the parameters of the material model that you select as design variables within the design space that you define. Therefore, the calibration requires the FE simulation to be robust enough to converge for all material parameters within the design space. Kinematically driven FE models are often more robust than load-driven models, especially in the presence of plasticity. Creating a completely robust simulation is often not possible; if a simulation fails to converge during a calibration with a given set of material parameters, the app attempts to adjust the parameters away from that region of the design space and continue with the calibration.
• Efficiency: During a calibration a simulation might be run hundreds or thousands of times. The more efficient you make your FE simulations, the faster the app can perform the calibration. Before you import a FE simulation, consider maximizing the efficiency of the simulation by prototyping and benchmarking. In general, the simulation models should have the fewest degrees of freedom (DOFs) possible while still ensuring accurate results. If applicable, you can minimize the number of DOFs by using axisymmetric and 2D simulation models. Mesh refinement studies can also help you find a good balance between accuracy and performance.
• Accuracy: The FE simulation model should be a good engineering approximation of the physical setup from which the test data was collected. Pay attention to prescribed conditions such as loads and constraints to ensure that they correspond properly to the actual conditions in the physical test.

Your imported FE models must satisfy the following specific requirements:

• All steps in your FE models must be general steps with nonlinear geometry enabled.
• Only static, quasi-static, and quasi-static implicit dynamic steps are supported.
• Each step must use automatic time incrementation. It is also suggested that you use the default minimum and maximum time increments for all steps in your FE models.
• You must ensure that the required node and/or element sets are defined in your FE model. The app can access response data from the simulation model only from a named node set that contains a single node or from a named element set that contains a single connector element.

FE Models With Multiple Steps

You can use an FE model with multiple steps. This approach enables you to calibrate a material response for a more complex workflow, such as performing a preloading step before you capture the test data. However, the app matches the response data to test data for an objective calculation from a single step that you select. If you have test data that you want to match to response data from multiple steps in the same FE model, import and match the test data for each individual step. You can match a single FE model to response data from any number of imported test data sets.

FE Models With Multiple Materials

You can include multiple material models in your FE model; however, the app can calibrate only one material definition from your FE model at a time. If you import an FE model that has more than one material definition, the app prompts you to specify the name of the material definition that you want to calibrate. During a calibration, the app overwrites the selected material model in the FE model with the material model you have defined within the app. For example, if your FE model has two materials definitions named Mat1 and Mat2, and you select Mat2 for the calibration, the app overwrites Mat2 and does not change Mat1.

The type of material model you select for Mat2 in the app does not have to be the same type of material model that was defined in the imported FE model. For example, suppose that Mat2 in the imported FE model was a simple linear elastic material. You define and calibrate Mat2 as an elastic-plastic material, a hyperelastic material, or as any other supported material model. You should confirm that the procedure type and element type in the imported FE model are compatible with the material model you select in the app. For example, if the FE model uses non-hybrid continuum elements, you cannot use this model to calibrate an incompressible hyperelastic material. In addition, if your FE model only includes static steps, you cannot calibrate a rate-dependent viscoelastic material.

Imported FE Models and Units

When you use FE models in a calibration, keeping track of units is important. It is good practice to set the units in the app before you import any FE models and to leave the units fixed for the session.

When you import a 3DEXPERIENCE simulation object from the database, the app converts its simulation units to the units currently specified in the Material Calibration app. The app stores the converted simulation locally for use during calibration. Once the import is complete, you cannot change the units in the local copy. If you need to run the calibration with a different set of units, reimport the simulation with a new set of units.

When you import an Abaqus input file, no conversion of units occurs. In this case, you should confirm that the units in the input file are consistent with the units set in the app and with the units of any other active FE model in the app.

You can specify any units when you define the material model in the app. When you launch a calibration or evaluation, the app automatically converts the material parameter values to the unit system you selected for the FE models.

Test Data and Data Matching

When you import test data for calibration while in FE mode, the primary goal is to import response data from the physical test that is compared against the simulation response during a calibration.

• You must include strictly monotonically increasing time data with every imported test data set. The app treats the imported time data as step time, which means it must always start at zero.
• You must also include at least one column of response test data to be used during a calibration. For example, if the test data is from a uniaxial tension test, the response data is typically either force or nominal stress.
• To minimize the overall calibration run time, your imported test data set should have the minimal number of points needed to capture the material response accurately.
• When you import test data, assign a label defining the units of the test data. You can import multiple columns of data; however, you can assign a specific label like Displacement only once in a test data set. If you need to import two or more column of the same type, import them in separate test data sets.
• After you have imported test data and the FE models, you can match columns of test data to simulation response output at the predefined single-entity node and connector element sets. The matched data set is available for the objective error calculations during a calibration.
• During test data matching, you can apply an optional scaling factor to the simulation response data. Applying scaling can make it easier to match test data to your FE response data. For example, suppose that for performance reasons you have created a quarter-symmetry FE model of a uniaxial tension test and are matching the uniaxial force in the simulation to the recorded force from a physical test. In this case, you might need set the scaling factor to 4.0 because the force in the simulation arising from a prescribed uniaxial displacement is be one-fourth of the force in the full model.
• Test data imported in FE mode is not available for calibrations using built-in simulation models.