This post describes a new calibration feature that became available in R2024x FD01, Feb 10, 2024 (on-cloud).

The image above comes from the Abaqus documentation for *CAP PLASTICITY

The Abaqus Benchmark manual problem "Limit load calculations with granular materials" was used as the source for this realistic Cap Plasticity material model for sand. 

Units are English: Inch, Pounds (lbf), psi.  You should change your display units, and your app units to these units. 

The Drucker-Prager/Cap model adds a cap yield surface to the modified Drucker-Prager model. The cap surface serves two main purposes: it bounds the yield surface in hydrostatic compression, thus providing an inelastic hardening mechanism to represent plastic compaction; and it helps control volume dilatancy when the material yields in shear by providing softening as a function of the inelastic volume increase created as the material yields on the Drucker-Prager shear failure and transition yield surfaces. The model uses associated flow in the cap region and a particular choice of nonassociated flow in the shear failure and transition regions.

The Cap Plasticity material model has been added to the 3DExperience calibration app only in the FE mode.  This is because FE models are typically required to enforce the modes of deformations commonly used in soils testing (triaxial tests).  The Cap Plasticity material model from this Benchmark manual problem was used to create six sets of synthetic test data:

1)  The limit load test

2)  A uniaxial compression test

3)  A confined compression test

4)  A "triaxal1" test : volumetric confinement followed by further uniaxial compression

5)  A "triaxal2" test : volumetric confinement followed by uniaxial unloading

6)  A volumetric compression test

All of the above Abaqus FE models are in units of inches, pounds, and psi.  All of the work in 3DX is shown in and calculated in these units. For all 6 models/tests, a known displacement is applied and a reaction force is measured. 

The image below is the starting point of an example calibration.  Some parameters were held fixed at their known value, while others were perturbed from their known value.  In the plots, synthetic test data is shown with symbols (solid circles) and the material model responses are shown as solid lines.  
 

The video below starts from scratch and shows the process of setting units, importing test data, importing a FE model, and then mapping between the FE output to the test data.  The parameters are perturbed from their known values and then a calibration performed. 

The image below is the known solution.  The material model snippet file, granularlimitload_mat_mod.inp, was imported into the calibration app and an Evaluation run.  Note the very small RSE error norms.
 

Known Solution (from the Benchmark manual problem)

** Units: English, Inch, Pounds, psi
**
*MATERIAL,NAME= SAND
*ELASTIC
30000.,0.3
*CAP PLASTICITY
16.212, 30.64, 0.1, 0.00041, 0.01, 1.0
*CAP HARDENING
  2.15, 0.0000
 20.96, 0.0005
 46.60, 0.0010
 79.67, 0.0015
126.28, 0.0020
205.95, 0.0025
311.27, 0.0028
655.60, 0.00299

The zip attached contains:

1) All of the synthetic test data in six different .txt files

2) The 6 Abaqus .inp files, units are inch, pound, psi.

3) A material model snippet file, named granularlimitload_mat_mod.inp

4) A 3DExperience file named Cap_Plasticity_Start.3dxml.  This requires version R2024 FD01 or later.

Back to:  Sharing Material Test Data

Back to:  Calibration examples, including narrated videos

Back to:  Material Modeling and Calibration - An Overview and Curriculum