If run an Abaqus FE simulation of a dogbone-shaped specimen pulled in tension, and you are using a PolyUMod material model, then you may see a strain distribution like the following. Everything looks great.
But if you then try to plot the plastic strain magnitude (called PEEQ in Abaqus), you see that the PEEQ variable is zero (0) everywhere.
So the question becomes:
How do you plot the viscoplastic strain magnitude when using the PolyUMod library?
For many of the PolyUMod material models the viscoplastic strain magnitude is automatically saved into state variable 2. So if you are an Abaqus user you will need a command like the following in your step definition:
*Output, field, variable=PRESELECT *Element output SDV
Here is the part of the PolyUMod User’s Manual that discusses the first 4 state variables:
Some of the recent material models in the PolyUMod library (for example the BB-model, the TN-model, and the TNV-model) do not calculate the viscoplastic strain magnitude by default. This decision was made in order to maximize the speed of the FE simulations. For these material models you need to specifically tell PolyUMod that you would like to also get the viscoplastic strain magnitude. You can do this by specifying that the PolyUMod global parameter 15 (called
FAILT) has a value of 16. Here is an exemplar TNV model that has this setting:
*User Material, constants=54 **..:....1....:....2....:....3....:....4....:....5....:....6....:....7....:....8 ** 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, 54, 43, 1, 500, 16, 0, ** NType1, NType2, NType3, FailT, C10, C20, C30, kappa1, 1, 2, 2, 0, 25, -1.25, 0.1, 750, ** kappa2, kappa3, C10, C20, C30, kappa1, kappa2, kappa3, 0, 0, 360, 0, 0, 750, 0, 0, ** tauHat, mm, bb, p0, fff, epsF, ceps, fss, 10, 8, 0, 0, 1, 0.1, 0.1, 1, ** C10, C20, C30, kappa1, kappa2, kappa3, tauHat, mm, 90, 0, 0, 750, 0, 0, 40, 8, ** bb, p0, fff, epsF, ceps, fss 0, 0, 1, 0.1, 0.1, 1
After FAILT has been set to 16, Abaqus will save the viscoplastic strain magnitude to SDV2 also for these material models. The following image shows that the viscoplastic strain magnitude has a max value of 0.344 in this example.
Viscoplastic Strain Magnitude in MCalibration
You can also plot the viscoplastic strain magnitude of the PolyUMod material models in MCalibration. To do this you need to select
FAILT=16 using the material model dialog box.
You can then plot state variable 2 also in MCalibration. The figure also shows that the viscoplastic strain magnitude is time-dependent, and often similar in magnitude to the applied total strain magnitude.