Compressibility

Abaqus/Standard has a special family of “hybrid” elements that must be used to model the fully incompressible behavior seen in hyperelastic materials. These “hybrid” elements are identified by the letter `H' in their name; for example, the hybrid form of the 8-node brick, C3D8, is called C3D8H.

Except for plane stress and uniaxial cases, it is not possible to assume that the material is fully incompressible in Abaqus/Explicit because the program has no mechanism for imposing such a constraint at each material calculation point. An incompressible material also has an infinite wave speed, resulting in a time increment of zero. Therefore, we must provide some compressibility. The difficulty is that, in many cases, the actual material behavior provides too little compressibility for the algorithms to work efficiently. Thus, except for plane stress and uniaxial cases, the user must provide enough compressibility for the code to work, knowing that this makes the bulk behavior of the model softer than that of the actual material. Some judgment is, therefore, required to decide whether or not the solution is sufficiently accurate, or whether the problem can be modeled at all with Abaqus/Explicit because of this numerical limitation. We can assess the relative compressibility of a material by the ratio of its initial bulk modulus, $K_0$, to its initial shear modulus, ${\mu }_0$. Poisson's ratio, $\nu$, also provides a measure of compressibility since it is defined as

Table 1 provides some representative values.

If no value is given for the material compressibility, by default Abaqus/Explicit assumes $K_0/{\mu }_0=20$, corresponding to Poisson's ratio of 0.475. Since typical unfilled elastomers have $K_0/{\mu }_0$ ratios in the range of 1,000 to 10,000 ($\nu =0.4995$ to $\nu =0.49995$) and filled elastomers have $K_0/{\mu }_0$ ratios in the range of 50 to 200 ($\nu =0.490$ to $\nu =0.497$), this default provides much more compressibility than is available in most elastomers. However, if the elastomer is relatively unconfined, this softer modeling of the material's bulk behavior usually provides quite accurate results. Unfortunately, in cases where the material is highly confined—such as when it is in contact with stiff, metal parts and has a very small amount of free surface, especially when the loading is highly compressive—it may not be feasible to obtain accurate results with Abaqus/Explicit.

If you are defining the compressibility rather than accepting the default value in Abaqus/Explicit, an upper limit of 100 is suggested for the ratio of $K_0/{\mu }_0$. Larger ratios introduce high frequency noise into the dynamic solution and require the use of excessively small time increments.