Problems about VUMAT in ABAQUS/Explicit.

[golfhigh]

I have some questions about VUMAT in ABAQUS/Explicit. Somebody kind familiar to it may give some good advice. Thanks.

subroutine vumat(
C Read only (unmodifiable)variables -
1 nblock, ndir, nshr, nstatev, nfieldv, nprops, lanneal,
2 stepTime, totalTime, dt, cmname, coordMp, charLength,
3 props, density, strainInc, relSpinInc,
4 tempOld, stretchOld, defgradOld, fieldOld,
5 stressOld, stateOld, enerInternOld, enerInelasOld,
6 tempNew, stretchNew, defgradNew, fieldNew,
C Write only (modifiable) variables -
7 stressNew, stateNew, enerInternNew, enerInelasNew )

Green-Naghdi stress is provided in VUMAT according to ABAQUS conventions. So it's believed both parameters of stressOld and stressNew should be located in Green-Naghdi frame.
Questions:
1. The parameter of strainInc is the Green strain increment in Green-Naghdi frame? Or anything else?
2. What time is the parameter of defgradOld relative to? The last incremental step relative to the initial configuation? The same question about another parameter defgradNew. Is it the present iterative step(not the present incremental step) relative to the initial configuation?

[Jorgen]

As they say "a dear child has many names", but the stress that Abaqus uses for the UMAT and VUMAT subroutines is according to their manuals the Cauchy ("true") stress. Check out both the user's manuals and the theory manual.

The issue about how to integrate rate-dependent material models is a separate topic. This is what the Abaqus manual has to say:

The Green-Naghdi stress rate is used when the mechanical behavior of the material is defined using user subroutine VUMAT. The stress rate obtained with user subroutine VUMAT may differ from that obtained with a built-in Abaqus material model. For example, most material models used with solid (continuum) elements in Abaqus/Explicit employ the Jaumann stress rate. This difference in the formulation will cause significant differences in the results only if finite rotation of a material point is accompanied by finite shear. For a discussion of the objective stress rates used in Abaqus, see “Stress rates,” Section 1.5.3 of the Abaqus Theory Manual.
If you haven't, check out Section 1.5.4 in the Theory manual.

The defGradOld variable is: "Deformation gradient tensor at each material point at the beginning of the increment."

- Jorgen

[golfhigh]

Dear Mr.Jorgen
Thanks for your reply.
I still have two questions in my mind:
(1)The defgradNew'notation-deformation gradient tensor at each material point at the end of the increment-is clear. I don't understand where it comes from, because the present incremental step is still not finished.
(2)Someone told me that the output stress is cauchy stress. What do you think? Do you konw how I can transform Green-Naghdi stresses to cauchy stresses using numercial method?
Thank you again.

[Jorgen]

(1) The deformation gradient at the end of the increment is indeed initially unknown. That is why the implicit finite element procedure is using a Jacobian and Newton iterations to find the equilibrium state.

(2) Yes, the output is Cauchy stress. How do you define "Green-Naghdi" stress? I know of "Green-Naghdi stress-rate", but I am not sure what you mean by "Green-Naghdi stress".

- Jorgen

[golfhigh]

Dear Mr.Jorgen
Thanks for your kind help!
Perhaps you didn't understand my true meaning. My questions:
(1)The deformation gradient at the end of the increment is indeed initially unknown. But I don't konw why it's provided in VUMAT parameters. I think it's unknown at the present step.

subroutine vumat(
C Read only (unmodifiable)variables -
1 nblock, ndir, nshr, nstatev, nfieldv, nprops, lanneal,
2 stepTime, totalTime, dt, cmname, coordMp, charLength,
3 props, density, strainInc, relSpinInc,
4 tempOld, stretchOld, defgradOld, fieldOld,
5 stressOld, stateOld, enerInternOld, enerInelasOld,
6 tempNew, stretchNew, defgradNew, fieldNew,
C Write only (modifiable) variables -
7 stressNew, stateNew, enerInternNew, enerInelasNew )

Is it a known parameter in vumat?

(2)The second question is about Green-Naghdi stress-rate in large deformation analysis. How I can transform it to the cauchy stress using numercial method?

[Jorgen]

(1) I still have some problems understanding what you are looking for. The deformation gradient at the end of the increment is provided in the variable defGradNew. That variable is needed in many models in order to perform the stress calculation.

(2) I don't understand what you are trying to do. You cannot convert a stress-rate into a stress. They have different dimensions!

- Jorgen

[golfhigh]

Hi Jorgen,

Recently I have been thinking over the questions. But I don't get any good conclusions. Conversely, I become more confused.

Do you kown the role of the stress rate? Someone told me to eliminate rigid rotations and keep the objective of stress-strain relations. What do you think?
In VUMAT I even don't see any shadow of the stress rate? Does that mean there is no need to consider the stress rate when we program VUMAT? Or the stress rate will play its role out of VUMAT?

I don't kown if I depict my questions clearly. Thank you for good advice.

[Jorgen]

The comment about "rigid rotations and keep the objective of stress-strain relations" is indeed correct. That, however, has nothing to do with the interface of the UMAT or VUMAT subroutines. You will need to keep that in mind as you develop a strategy to ingrate your constitutive model inside the user material subroutine. It is up to you to make sure your subroutine is objective.

- Jorgen