I am working on a problem that requires estimating the amount of rate dependency the material should have in order to perform as per the given specs under a rapid dynamic load. For this, I am looking for a finite (large) strain viscoplastic model, something like: A (\sigma) + B (\sigma_dot) = C (\epsilon) + D (\epsilon_dot)
I want to be able to vary the coefficients A,B,C, and D to study the effect of rate dependency on the results.

I have these questions:

Is the “incremental viscoplastic model with multiplicative decomposition” of CalculiX the right choice for this kind of problem?

Is there a similar model in ABAQUS?

How is using “*RATE DEPENDENT different than using *CREEP” with *PLASTIC in ABAQUS/CalculiX?

What is the difference between time hardening and strain hardening? I understand what strain hardening is: “that accumulation of dislocations near grain boundaries, restricting further motion, hence increasing yield limit after unloading–> reloading”, but what is time hardening? Is it the time dependency of strain rate on time t as in Norton Law? Just that or more, I mean physically?

What kind of material do you want to model ? Can you say more about it ? According to the documentation, CalculiX uses standard additive decomposition when *PLASTIC and *CREEP is specified but NLGEOM is off. With NLGEOM on it switches to multiplicative decomposition. Maybe you will need something more specific and thus UMAT will become necessary.

In Abaqus multiplicative decomposition is used only in the permanent set model which is meant for polymers and used with hyperelasticity. Otherwise, you would have to write UMAT.

CalculiX doesn’t have the *RATE DEPENDENT keyword so I will focus on Abaqus here. In both cases, there’s a rate dependency but *RATE DEPENDENT is just an addition of the dependency of yield strength on strain rate for various plasticity models (including Johnson-Cook for example). Creep is a more specific phenomenon described by separate laws.

This choice is given in Abaqus, in CalculiX there’s only one creep model and others have to be implemented via CREEP subroutine. The time hardening model is the simplest one and is equivalent to what CalculiX offers. The strain hardening model is more complex. Check their equations in Abaqus documentation (chapter “Rate-Dependent Plasticity: Creep and Swelling”).

Like I said earlier, something like: A (\sigma) + B (\sigma_dot) = C (\epsilon) + D (\epsilon_dot)
I want to be able to vary the coefficients A,B,C, and D to study the effect of rate dependency on the results.
Plus, the model should be valid for large plastic strains. Because in ABAQUS/CalculiX, by default *PLASTIC calls J2 plasticity which is a small strain theory, right? If I use the NLGEOM option, does ABAQUS/CalculiX use a large/finite strain theory instead of the small strain J2 plasticity theory?

(Also, I am only looking at single shot loading and no unloading. Meaning a hyperelasticity-based material might also work so long as it has rate dependence, something like visco-hyper-elastic)

I was rather referring to the type of material that you want to model - if it’s metal, polymer, composite or something else and possibly more details about it.

The regular elasto-plastic model should be fine even for large plastic strains unless you want to account for nonlinear elasticity and simultaneous presence of both elastic and plastic deformation from the beginning (that’s where multiplicative decomposition would become useful).

Abaqus also offers a very advanced and complex nonlinear viscoelastic-elastoplastic PRF (Parallel Rheological Framework) model that can be used (potentially in conjunction with other models such as the Mullins effect) to accurately represent the behavior of various polymers.

There are many material models (and their number is still growing) for very specific applications but they all need good test data and that’s where you should start. If you can perform various physical tests then it’s just a matter of calibration to obtain the constants for different models.

Interestingly, CalculiX even offers an anisotropic hyperelasticity model, developed by Holzapfel and meant primarily for artery walls. Unfortunately, CalculiX doesn’t have time and frequency domain viscoelasticity models where Prony series coefficients, creep/relaxation test data or storage/loss moduli are used (those are available in Abaqus though).

Oh sorry, I misunderstood previously.
The material is actually metal foam. And for that, there is this “crushable foam model” in ABAQUS.

But I actually want to explore the whole range/family of foam-like materials (involving rate dependency which “crushable foam model” in ABAQUS does not include) by doing an inverse study (if I can say so). Meaning I have my design requirements/performance metrics for say a given loading condition and I want to find out which material out of this family of materials meets these requirements (that’s where those coefficients A,B,C,D come in).
I hope this gives a clear picture.

I had no idea about this. Thanks for this. This might turn out to be relevant.

For my particular case, although foam-like materials have some level of anisotropy; but given that it is highly random, the assumption of isotropy holds. Or at least, I am making this assumption for my problem.
So isotropic model is also fine for me. But thanks for this.

Both Abaqus and CalculiX also have a hyperfoam material model if you want to account for nonlinear elasticity. CalculiX doesn’t offer the crushable foam model but it would be interesting to see its implementation via UMAT. Subroutines open up many possibilities in terms of material modeling but they require quite a lot of work and literature studies.

The Hyperfoam model both in ABAQUS and CalculiX, is a non-viscous model, meaning no rate effects can be captured, right?
Found the following note on the Hyperfoam page:

So I looked into this Low Density Foam model which is defined as a pseudo visco-hyperelastic model (doc image below) that can be used to capture the rate effects. (WebPage: Low-density foams)

I believe this model can work for my problem, but I want to check the complete details of it which are not available on the doc page that I’ve hyperlinked above.

Has anyone used this model? Can I get the full details of this model? I mean the equations. Or is there a research paper on which this model is built?

Yes, it’s just a form of nonlinear elasticity (hyperelasticity) that assumes high compressibility (while regular hyperelastic materials such as rubbers are almost incompressible). In fact, it’s a modified version of Ogden hyperelastic model.

I haven’t used it and the Abaqus documentation doesn’t refer to any research papers in which it was introduced. Maybe check the LS-DYNA Theory Manual, they use similar models and provide the equations and references to literature for them.