Calibrate a PolyUMod Material Model with Failure

The goal of this tutorial is to show how you can calibrate both a non-linear viscoplastic PolyUMod material model and a strain-rate dependent failure model using MCalibration. In the specific example shown here, I will calibrate the PolyUMod TNV model to the experimental data shown in the figure to the right. See the following post for more information about this specific experimental data set.

This type of calibration requires 2 steps: (1) first calibrate the stress-strain predictions, (2) calibrate the failure model (while keeping the stress-strain parameters constant). This article summarizes the key steps. All details of all steps are presented in the following YouTube movie.

The figure to the right shows the final predictions after calibrating the stress-strain model. The average error in the model predictions is about 2%, which is quite good.

To calibrate the failure model parameters we first deactivate optimization of the parameters that control the stress-strain response, and then activate the parameters that control failure.

This figure shows the failure model parameters that will be optimized. Note that I selected failA=0.01, and failB=0.1 based on the experimental strain rates.

To facilitate the parameter optimization I also recommend setting a Failure Time in the load case setup dialog. Note that you should deactivate all load cases that are not taking the specimen to failure.

The results from the final stress-strain predictions, including failure, are shown in the following figure. The calibrated material model captures all aspects of the experimental data accurately.

To use this material model in an Abaqus simulation than includes element deletion you also need to activate the element deletion flag in the Material Model dialog box.

The final material model parameters are summarized below, and all details of the steps summarized here are demonstrated in the following movie. The movie also shows how you can use the calibrated material model in an Abaqus/Explicit FE simulation that includes element deletion.

					*Material, name=Mat
** Units: [length]=millimeter, [force]=Newton, [time]=seconds, [temperature]=Kelvin
** Material Model: PolyUMod-TNV
*User Material, constants=74
**     MM,      ODE,      JAC,     ERRM,   TWOD_S,     verb,    VTIME,    VELEM,
       29,        0,        3,        0,        0,        1,        0,        0,
**   VINT,   ORIENT,    NPROP,    NHIST,      GMU,   GKAPPA,    FAILT,    FAILV,
        0,        0,       74,       43,        1,      500,        0,        0,
** NType1,   NType2,   NType3,    FailT,      C10,      C20,      C30,   kappa1,
        2,        2,        4,        1,    2.944,        0,        0,       80,
** kappa2,   kappa3,   tauHat,       mm,       bb,       p0,      fff,     epsF,
        0,        0,  2.04563,    2.433,        0,        0,      0.2,   0.0753,
**   ceps,      fss,      C10,      C20,      C30,   kappa1,   kappa2,   kappa3,
     1.08,    1.546,     6.05,        0,        0,       80,        0,        0,
** tauHat,       mm,       bb,       p0,      fff,     epsF,     ceps,      fss,
     3.66,       20,        0,        0,     2.04,   0.0154,   0.0369,    0.302,
**    C10,      C20,      C30,   kappa1,   kappa2,   kappa3,        r,     Uhat,
     1.17,        0,        0,       80,        0,        0,     2.02,     0.07,
**   beta,       FF,       GG,       HH,       LL,       MM,       NN,failStrai,
        0,        1,        1,        1,        1,        1,        1,0.9724183,
**failStr,    failA,    failB, failTAx1,   failF1, failTAx2,   failF2, failTAx3,
0.9533748,    0.001,      0.1,        0,        1,      0.3,        1,      0.6,
** failF3,failDStra
        1,     0.02
*Depvar, delete=4
1, Sim_Time
2, ViscoPEEQ
3, E1
4, FailFlag
5, ERate
39, MaxSTR
41, RISC

Share on facebook
Share on twitter
Share on linkedin

More to explore

Leave a Comment