Mooney Rivlin model

[Wei]

Hi All,

I have a question regarding the Mooney Rivlin model,

Say W=C10*(I1-3)+C01*(I2-3), where I1 and I2 are strain invariants, C10 and C01 are material constants

The corresponding second Piola-Kirchhoff stress is

S=2*((C10+C01*I1)*I-C01*C), where I is the identity tensor and C is the right Cauchy-Green strain tensor.

So the component of S, say, S11=2*(C10+C01*I1-C01*C11)

If material is isotropic and no shear, so I1 can be expressed as C11+C22+C33

Then S11=2*(C10+C01*(C22+C33)) which is always >=2*C10. Does this violate the concept that at reference configuration, W and S should be zero?

Appreciate any help to explain this.

Wei

[Jorgen]

Hello Wei,

You write that

The corresponding second Piola-Kirchhoff stress is

S=2*((C10+C01*I1)*I-C01*C), where I is the identity tensor and C is the right Cauchy-Green strain tensor.

This is not quite right. Your are missing the term: -p C^{-1}, where p is the indeterminate pressure due to your incompressibility assumption in the strain energy function. For more info, see e.g. Holtzapfel's "Non-linear Solid Mechanics" p. 224.

Jorgen

[Wei]

Hi Jorgen,

Thanks for the reply.

You are right that for incompressible material
S=2*((C10+C01*I1)*I-C01*C)+pC^(-1) (1)

When one needs to fit experiment data to the equation to determine material constants, it appears to me that one only needs to use
S=2*((C10+C01*I1)*I-C01*C) (2)

to fit. Apparently eqn(2) can not fit the experiment data. I notice in ABAQUS nominal stress and stretches are used to fit, however, when coding in UMAT, eqn(1) is used. How to directly use either (1) or (2) to fit the data to obtain material constants? presume that I have experimental S, I1 and C.

Thanks again,

Wei

[Jorgen]

Hello Wei,

If I wanted to find the material parameters from uniaxial tension or compression data, I would use Eq. (1), while keeping p as a Lagrange multiplier. You can find p, for example by considering that the transverse stresses are zero in uniaxial loading. Note, the pressure p will likely be a function of the applied strain. In fact, you should be able to solve for p this way and come up with an expression for the uniaxial stress as a function of the uniaxial strain and the material parameters. Once you have that expressin you can easily find C10 and C01. Also, I suspect that the ABAQUS theory manual outlines the needed expressions for the M-R model.

Jorgen

[Wei]

Hi Jorgen,

One more question related to the UMAT code of Neo-Hookean materal model. Can the DDSDDE be the elasticity tensor in spatial description defined in Holzapfel's "nonlinear solid mechanics" pg265? It appears to me that they are not the same, based on the UMAT code provided by ABAQUS and the formulation in the book. Do you know what is the relationship between the elasticity tensor and DDSDDE?

Thanks for your help,

Wei

[Jorgen]

Wei wrote:
I guess I found the answer in the book "Nonlinear Finite Element for Continua and Structures" by Belytschko. If the tangent moduli of Jaumann rate of Cauchy stress is used for DDSDDE, then according to Eqn (5.4.27) of the book, the tangent moduli of Jaumann rate of Cauchy stress C{J)=C{T}+C{*}, and C{T}=J^(-1)*C{t} by Eqn (5.4.51). C{t} is the fourth elasticity tensor by Eqn(5.4.50). Since I know C{t}, the I can get C{J} backwords from above equations, is it correct? I will code it in and compare with the UMAT ABAQUS provided.


Your approach seems OK. I suggest that you go ahead an give it a try.
Here's another, perhaps less elegant, approach: approximate DDSDDE using a finite difference approach. I have had good success with this approach, both in terms of the time required to code the subroutine and the actual run time; especially for advanced viscoplastic models.

Jorgen

[Wei]

Hi Jorgen,

Thanks for your reply!

Do you have any reference on the finite difference approach and on how to implement it in FE?

To approximate the elasticity tensor numerically, the only work I know is by Dr. Miehe on Comput. Methods Appl. Mech. Engrg. 134(1996) 223-240. However, in that paper, the deformation gradient is the primary variable for the perturbation process. I wonder if the method will work for a load-control simulation. I wonder by your experiences if an approximating algorithm can be the same for both load-control and displacement-control simulations.

Thanks again and have a nice weekend,

Wei

[Jorgen]

I don't yet have any reference on the implementation details :(
I have been thinking about writing something up about it, but I have not had the time.

The numerical approach to determine the Jacobian works equally well for load control and displacement control.