The main motivation for implementing FE mode in the calibration app is to deal with tests in which the stress/strain field is non-homogeneous (gradients exist in the measurement region). Easy example: spherical indentation of a foam material. Or any test in which the material undergoes damage / failure. In these cases, a calibration can be carried out only if a multi-element FE mesh/model is used to faithfully mimic the test conditions and gradients. This Makrolon example is a bit different from that case. In analytical mode and numerical mode we assume the time and strain are known and the stress response is needed. But in creep testing the time and stress are known and the strain is the unknown/measured quantity. So, we use FE mode to work around this limitation of numerical mode.
This post was originally written using a development version of R2021x FD05.
The test data is creep data at 5 different stress levels.
The target material model is "Elastic-Creep".
This calibration can be performed using the standard numerical mode (no FE model), but the app always assumes that
Result of the numerical mode calibration:
For the FE-based calibration, switch to FE-based mode before importing any test data.
General set of steps:
1) Switch to FE-based mode of calibration.
2) Import test data.
3) Import one or more FE mesh/models.
4) Map the particular FE output to be compared to a particular test data set.
5) Select the material model.
6) Use the "Evaluate" feature to show a one-time comparison using the current model parameters. Possibly adjust parameters by hand and re-run "Evaluate".
7) Run the calibration.
The FE-based calibration tool thinks that the FE output will be history output of things like force, moment, displacement, rotation.
In this example, the FE unit-cube models output U3 and TF3, but because of the unit-cube, these quantities are the same as nominal strain and nominal stress. All of the FE model output is for the single-node nset named "LoadPt". We map like this:
Video of FE-based calibration. This worked ok when I made the video below. Later in time (R2022x) a bug crept into things. IR-905364 "For a particular analysis using a *VISCO procedure, Abaqus/Standard omits to provide output at user specified time points". This was fixed in a later release of R2022x and all versions going forward.
Limitations for FE mesh/model usage:
1) Any input file used with the FE calibration must be flattened. "parts & assembly" style models cannot be used.
2) It only supports *STATIC, *VISCO and *DYNAMIC, IMPLICIT analyses.
- *STATIC cannot have the DIRECT parameter
- *VISCO must have the CETOL parameter
- *STEP cannot have PERTURBATION parameter
3) The FE output that you want to compare against the test data must be in a single-node nset and things like U, RF, TF. You may also use a single-element elset for use of connector element output.
4) The input file should not contain parameters.
5) Only support solid, shell, and beam sections for calibrated material.
6) Multiple materials are allowed, but can only calibrate one of them.
7) 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.
8) 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.
9) If the run-ready model is imported as an input file (.inp), the units embedded in this file must be respected.
In 2020x FD04 this feature is hidden behind the environment variable
SMAMATCAL_MESHEDCALIBRATION
Test Data in Excel:
The 5 FE unit-cube input files in a singe zip file:
Back to: Sharing Material Test Data
Back to: FE-based Material Model Calibration
Back to: Calibration New Features in R2021x FD05
Back to: Material Modeling and Calibration - An Overview and Curriculum
