# Incompressible Material Models

I’m behind the calculation of the Strain Energy Density of some material models to compare with ccx ENER.

As a first attempt the models under consideration are the same ones I have used to check the NEO HOOK and Money-Rivling material model on the post: Hyperelastic Pipe - #43 by Disla.

In order to simplify my calculations, I have modify D1 parameters in such a way that the material models are nearly incompressible , so that J=1 and the volumetric part of the Strain Energy vanishes. This way I can focus first on the deviatoric part of the Strain Energy density.

Hyperelastic models are appropriate for comparison up to a maximum of 300% strain so that has been my first set up.

No matter which model is under consideration , I have noticed that they are all changing their volume from the first beginning up to a considerable amount ( 20% in my particular study case) although they are defined as incompressible.

Ccx 2.19 and ccx 2.20. I have compute with C3D20R hex elements because manual says full integration are bad for isochoric material behavior.

¿Isn’t volume change on Incompressible hyperelastic models = 0?
¿Should I expect the same error in the Strain energy density value?

Quote from CalculiX User’s Manual:

Perfectly incompressible materials require the use of hybrid finite elements, in which the pressure is taken as an additional independent variable (in addition to the displacements). CalculiX does not provide such elements. Consequently, a slight amount of compressibility is required for CalculiX to work. If the user inserts zero compressibility coefficients, CalculiX uses a default value corresponding to an initial value of the Poisson coefficient of 0.475.

Abaqus offers hybrid elements but in explicit analyses full incompressibility cannot be used.

Ohh, thanks Calc_em,

I’m not sure if I understand this properly.

CalculiX makes use of hyper-elastic material models which are virtually incompressible.
To implement this material models, one needs hybrid finite elements which are not available.
To solve this one must consider some compressibility. A value for the Poisson Ratio of 0.475 is set as maximum default regardless of the coefficient (1/D1) that controls the compressibility in such models.

Rubbers have Poisson ratios between 0.48 - 0.5. ¿How could this be overcome ?

EDITED: Sorry I didn’t want to lose the opportunity to ask this. It just came to my mind a note on the manual.

In the present implementation of(visco)plasticity the Plastic ﬂow is isochoric (the volume is conserved).
Is this the reason why full integration elements are said to behave badly?
¿How do we solve this incompressibility if there are not suitable elements for this?.

Thanks

This default value is used only when the compressibility coefficients are specified as zero.

In Abaqus/Standard (implicit), hybrid elements have to be used for incompressible and nearly incompressible (PR>0.495) materials (although it’s possible to remove this restriction for materials that are not fully incompressible) and should be used for other approximately incompressible materials to improve convergence. In Abaqus/Explicit, except for plane stress and uniaxial cases full incompressibility is not allowed. If compressibility is not specified, the solver assumes PR=0.475.

Of course, the lack of hybrid elements in CalculiX can be problematic but many cases should be solvable without them.

Elements with full integration may exhibit volumetric locking behavior in analyses involving hyperelasticity or plasticity with high plastic strain (> 10%). Hybrid elements are indeed a way to mitigate this problem.

I wonder if CCX is using poisson’s ratio = 0.475 when D1 is within some threshold of zero and your value (1e-7 mm^2/N = 1e-14 m^2/N) is so small that it’s treated as zero. The value shown in Mecway only uses 0.475 for D1=0 exactly. So maybe you can increase it by using a bigger D1?

You nailed it Victor.
In fact, this solution was also in between Calc_em lines :

Sorry to insist again but I think you MECWAY should consider exporting INP files in SI(mm).

Thank you very much both. I can keep going with the Strain Energy.