Basic VUMAT question

[sq]

I've coded linear-elastic and neohookean VUMATs that start with the deformation gradient [F]. I've been using [F] because my linear elasticity model is based on the strain measure [E] = ln [V].

These models have been successfully tested in single-element simulations. However, at long integration times, interesting numerical stability problems start to occur. I wonder, could this be a consequence of starting with the [F] rather than with the right symmetric stretch tensor [U], as suggested in the ABAQUS User's guide?

Ordinarily, I'd think not, one should follow from the other, but I seem to be encountering a case where a small perturbation is growing in an unbounded way, leading to aphysical displacements in the result (after a deformation and recovery event).

[Jorgen]

Here are few comments/suggestions:

:arrow: It is typically recommended to use the tensor U instead of F when coding a VUMAT. The simple reason for this is that it is easier since that way the rotations will be correctly accounted for. If you use the tensor F then you need to make sure that you do the appropriate rotations.
:arrow: Do you see the numerical instabilities also for simple uniaxial tension?
:arrow: Do you see the numerical instabilities at the same time for both single precision and double precision runs?
:arrow: Is it possible that the instabilities are due to numerical round-off issues and not F vs. U?
:arrow: Have you verified that you implementation works for a case with finite rotations such as simple shear?

Best of luck,
Jorgen

[sq]

Jorgen,

Many thanks for these ideas. The model is indeed accurate and numerically stable for uniaxial and simple shear trial cases. I like your thoughts about double precision/roundoff error - I was worried about small (but nonzero) perturbations propagating through the solution. I think I'll give the dp version a try.

[sq]

Okay, maybe the last bullet was most important.

I included in my "test cases" a larger simple shear numerical experiment, and the whole thing fell apart. The lesson here seems to be that I am indeed having a problem when finite rotations are present.

The trouble is, most of my stress formulations have been in the left-symmetric matrices (i.e., V and B), rather than in U, which ABAQUS provides directly. I thought I was doing a decent job of getting V from F by finding the eigenvalues through Jacobi iteration, but I must be missing something.

[sq]

Rats - it turns out my problem was even more basic than that. Let this be a warning to those using VUMATs in ABAQUS where large rotations may occur- you will probably need to rotate your stress tensor, as ABAQUS requires that "the constitutive model is defined in a corotational coordinate system in which the basis system rotates with the material".