A singleprecision Abaqus VUMAT subroutine for the NeoHookean (NH) model. The subroutine is an example of how to write a VUMAT. The subroutine only works for planestrain, axisymmetric, and 3Delements.
Announcement
Collapse
No announcement yet.
ABAQUS VUMAT for the NeoHookean model
Collapse
X

VUMAT condition
Hello Dr;
You below the condition that I applied to initialize the FE that correcpond in my simulation gradien elastic.
Abaqus compile when I got started in the calculation and stops immediately, and when I calculate this condition normally, but on this condition is necessary to get good results.
So is what you think is the right way to proceed?
IF (totTime.EQ.0.0) THEN
C setup FE (upper diagonal part)
FE(1,1) = 1.02
FE(2,2) = 1.039
FE(3,3) = 1.059
FE(1,2) = 1.079
if (nshr .eq. 1) then
FE(2,3) = 0.0
FE(3,1) = 0.0
FE(2,1) = 0.0
FE(3,2) = 0.0
FE(1,3) = 0.0
else
FE(2,3) = 1.0099
FE(3,1) = 1.029
FE(2,1) = 1.0049
FE(3,2) = 1.079
FE(1,3) = 1.809
end if
END IFdoctorant polymer
Comment

The flow equation that you mention actually work rather well for many different types of polymers. Abaqus has two a model called "Two layer viscoplasticity" that I believe supports that flow rule. I have not had much luck with that model, however.
Another approach is to use the *Hysteresis model in Abaqus. That model is also based on that flow rule.
A third option is to write your own usermaterial.
 JorgenJorgen Bergstrom, Ph.D. PolymerFEM Administrator
Comment

Ok once again i posted too quickly by searching in the archives i found some interesting post i have to understand first.
My understanding is that anything rigid body is controlled by abaqus explicit if one wants by using U, and it is equivalent to F and V in this framework.
original message:
Dear Jorgen. I am trying to understand this vumat before wirting my own (TNM based). But i am struggling at one point.
By going backward in the code.
I am all ok for:
c Stress = mu/J * Dev(Bstar) + kappa*log(J)/J * Eye
and for
c Bstar = J^(2/3) F Ft (upper diagonal part)
But my feeling by reading the code is that instead of calculating F Ft you take the square of the stretch tensor. I would have no problem with that if ABAQUS was proposing the left stretch tensor ( F = V*R => F * Ft = V* R * Rt * Vt = V² V being symmetric) but i read ABAQUS documentation and it says that VUMAT communicate the RIGHT STRETCH TENSOR F = R * U !
So i don't understand something. Can you explain ?
By the way the ABQ doc says that the user should use U instead of F to write hyperelastic law but i don't really see how.Last edited by Ajaj; 20121102, 07:42.
Comment

Originally posted by Ajaj View PostOk once again i posted too quickly by searching in the archives i found some interesting post i have to understand first.
My understanding is that anything rigid body is controlled by abaqus explicit if one wants by using U, and it is equivalent to F and V in this framework.
original message:
Dear Jorgen. I am trying to understand this vumat before wirting my own (TNM based). But i am struggling at one point.
By going backward in the code.
I am all ok for:
c Stress = mu/J * Dev(Bstar) + kappa*log(J)/J * Eye
and for
c Bstar = J^(2/3) F Ft (upper diagonal part)
But my feeling by reading the code is that instead of calculating F Ft you take the square of the stretch tensor. I would have no problem with that if ABAQUS was proposing the left stretch tensor ( F = V*R => F * Ft = V* R * Rt * Vt = V² V being symmetric) but i read ABAQUS documentation and it says that VUMAT communicate the RIGHT STRETCH TENSOR F = R * U !
So i don't understand something. Can you explain ?
By the way the ABQ doc says that the user should use U instead of F to write hyperelastic law but i don't really see how.
Hi Ajaj,
I had the same question a while ago  I think this document would answer your question regarding using U^2 instead of V^2.
http://imechanica.org/files/appendix3vumat.pdf
page A3.29.
Due to the corotational frame, you are actually calculating the corotational portion of the Cauchy stress:
sigma = R * sigma_corot * Rt
using the corotational portion of the left CauchyGreen deformation tensor:
B = F * Ft = R * U * Ut * Rt = R * U^2 * Rt
Comment

Quick question for everybody !
Why a high Bulk modulus over shear modulus ratio leads to high kinetic energy in an Explicit analysis and unstable results ?
I'm using Dr. Bergstrom's subroutine (NeoHookean) to model indentation. I works and I'm really thankful as this subroutine helped in understanding the basic process of using a typical VUMAT.
However the elements under the indenter which suffer high compression start distorting and the analysis stops. The builtin NeoHookean doesn't show this problem.
The higher the Bulk modulus over shear modulus ratio, the smaller the strains at which the distorsion occurs. However the kinetic energy becomes significant even for little mass scaling.
I would be glad if someone can explain the mechanism that triggers that and also discuss about what the example subroutine provided may be missing.
Thanks
Christos
Comment
Comment