Pore Fluid Pressure

In geotechnical applications a porous medium typically consists of a solid skeleton of numerous solid grains that are “loosely packed” and a pore fluid that flows through a system of interconnected pores among these solid grains. When subjected to loading, both the solid skeleton and the pore fluid respond in a manner that leads generally to a fully coupled response where the deformation in the solid skeleton depends on the pressure of the pore fluid and vice versa. Abaqus/Standard supports analysis of such a porous medium through a fully coupled pore pressure–displacement analysis (see Coupled Pore Fluid Diffusion and Stress Analysis).

In some situations you can approximate the two-way coupling using a sequentially coupled approach that consists of the following two parts:

1. A purely pore fluid flow analysis that computes the pore fluid pressure distribution in the porous medium without accounting for the deformation in the solid skeleton. Typically, third-party software is used to complete this part (outside of Abaqus).
2. A pure stress analysis that computes only the deformation of the solid skeleton, taking into account the effects of the pore fluid pressure field computed in the first part. Typically, a static or explicit dynamic analysis in Abaqus is used to complete this part.

The pore fluid pressure definition allows the inclusion of a known pore fluid pressure field as a predefined field variable in Abaqus in the second part of the sequential workflow above (see Predefined Fields for Sequential Coupling). The material constitutive response in the stress analysis is defined in terms of:

• the behavior of the solid skeleton, which can utilize any of the mechanical constitutive models available in Abaqus, and
• the known pore fluid pressure field computed in the first part of the sequential analysis and included in the second part as a predefined field variable.

The pore fluid pressure, $u_w$, contributes to the total stress as

In the above expression $\mathit{\sigma }$ is the total stress, and ${\overline{\mathit{\sigma }}}^{*}$ is the effective stress that is a function of the effective strain and the constitutive response of the solid skeleton (see Effective stress principle for porous media). A static stress analysis in Abaqus/Standard can account for the compressibility of the solid grains (see Porous Bulk Moduli) in computing the effective strain by subtracting the volumetric strain in the solid grain due to the pore pressure from the total strain. An explicit dynamic stress analysis in Abaqus/Explicit assumes that the solid grains are incompressible and that the effective strain is equal to the total strain.

MATERIAL, NAME=name
PORE FLUID PRESSURE, FIELD=n

To initialize the known pore fluid pressure field, you must initialize the corresponding field variable.

INITIAL CONDITIONS, TYPE=FIELD, VARIABLE=n