R2021x FD05 is a major new release for the 3DX Materials Calibration app.
A variety of new features were released with R2021x FD05, aka FP2108. That version was released for on-premise on Feb 26, 2021. The public cloud upgraded on Saturday, March 13, 2021, called HotFix 5.7. By Monday night, March 15, it was called HotFix 5.9. See the SIMULIA documentation, Whats New, for the calibration app.
This post explains a bit about using the FE-based calibration and contains several examples. FE models are required for calibration of damage and failure models. Another example where they are required is for any experiment in which the state of stress/strain is non-homogeneous, such as in indentation testing, There are also times where the FE-based calibration can be used with a simple unit-cube (1 element) mesh to overcome a limitation in the analytical or numerical modes.
You can visit these examples, but you might want to finish reading this post first.
Examples:
3DX FE mesh/model calibration of the rubber puck (uses 1 Abaqus model)
Video created using R2021x FD05. This is a good example to try first, because the FE model is axisymetric and quite small, the FE model runs in just a few seconds, so it keeps the calibration time low.
Necking of a titanium dogbone specimen (uses 1 Abaqus model)
Video created using an earlier development version of 3DX.
Makrolon Creep Example ; using FEA unit-cube models (uses 5 Abaqus unit-cube models)
Video created using an earlier development version of 3DX. Needs a refresh.
FE-mode simple elastic calibration w/ unit cube (uses 1 Abaqus model, with a single element)
Video created using R2022x FD02 on April 26, 2022.
FE-mode simple elastic calibration w/ two materials (uses 1 Abaqus model, two materials)
Video created using R2022x FD02 on May 18, 2022
Comparing A/CAE, Analytical mode, Numerical mode, and FE mode calibration
This example uses 1 Abaqus .inp file, but contains 3 separate unit cube FE models.
Video created using R2022x FD02 on May 2, 2022
General Process: The general idea is that the user supplies a 'run-ready' Abaqus model that replicates the test physics. This model can be created in the 3DX platform, or imported as an Abaqus input file (.inp).
Working from left to right in the icons above:
1) Switch to FE-based mode. Once you do this you will notice that the icons change a bit.
2) Import test data. In this 1st release we have focused on importing test results like force/moment and displacement/rotation. We do support importing stress and strain, but there are limitations on how you will match this against the FE results.
3) The icon for 'Range Response Data' (aka Response Only data) has been removed.
4) Use the Import Mesh icon to import your run-ready Abaqus model. The app supports the use of multiple FE models.
5) Use the Meshed Output icon to map, or match, the various pieces of test data to the corresponding FE model output.
6) Select your material model. Only one material model may be calibrated.
7) Run a one-time Evaluate of the model using the current material parameters. This step is to check that everything is working and that the current material parameters give a response that is at least in the right ballpark.
8) Execute a calibration
FE-based mode limitations:
1. An imported Abaqus .inp file must be “flattened”, no parts & assemblies are allowed.
2. The app only supports A/Std and only *STATIC, *VISCO and *DYNAMIC, IMPLICIT steps.
- *STATIC cannot have the DIRECT parameter
- *VISCO must have the CETOL parameter
- *STEP cannot have PERTURBATION parameter
3. FE output must be from single-noded nsets or single-element elsets.
- a single-element elset must contain a connector element.
4. The input file's material to be calibrated should not contain parameters. The calibration app will overwrite the calibrated material, and constructs like this will be lost
*Parameter
C10 = 1.0
C20 = -0.1*C10
C30 = 0.01*C10
D1 = 0.001
*Material, Name=Elastomer
*Hyperelastic, Yeoh
5. Multiple materials are allowed in your model, but can only calibrate one of them.
6. Only support solid, shell, and beam sections for calibrated material.
7. Be careful with units
- For Abaqus .inp file imported, the app knows nothing about those units.
- The user is fully responsible for making sure the correct units are used for the calibration.
8. The step time for a step containing matched output requests will be extended if the step time is less than the total time for one of the matched tests. The step time will never be shortened to match test time, just extended.
9. If there are steps in the original input file after the last step containing matched output requests, these steps will be removed from the analysis as they do not contribute to any calibration results.
10. Be careful about your model's run-time. This is not a limitation of the app, but just a fact of life. The calibration optimizer will have to run your model many times, so the performance of your model will dictate the time it takes to perform the calibration. Care should be taken to create a small model.
Back to : Calibration New Features in R2021x FD05
Back to: New Material Model Calibration App in 3DEXPERIENCE Platform
Back to: Material Modeling and Calibration - An Overview and Curriculum
