You can define specific properties for a fluid-filled porous material. This type of porous medium is considered in a coupled pore fluid diffusion/stress analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1 of the Abaqus Analysis User's Guide). In addition, permeability is considered in an Abaqus/CFD analysis (“Incompressible fluid dynamic analysis,” Section 6.6.2 of the Abaqus Analysis User's Guide).
For detailed instructions, see the following sections:
You can model the growth of gel particles that swell and trap wetting liquid in a partially saturated porous medium. For more information, see “Swelling gel,” Section 26.6.5 of the Abaqus Analysis User's Guide.
To define a swelling gel:
From the menu bar in the Edit Material dialog box, select Other
Pore FluidGel.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Enter the following data in the Data table:
r_a(dry)
Radius of gel particles when completely dry, 
. (Units of L.)
r_a(f)
Fully swollen radius of gel particles, 
. (Units of L.)
k_a
Number of gel particles per unit volume, 
. (Units of L–3.)
tau_1
Relaxation time constant for long-term swelling of gel particles, 
. (Units of T.)
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
The Edit material dialog box allows you to define the saturation-driven volumetric swelling of the solid skeleton of a porous medium in partially saturated flow conditions. You can use this type of material definition in the analysis of coupled wetting liquid flow and porous medium stress. See the following sections for more information:
To define moisture swelling:
From the menu bar in the Edit Material dialog box, select OtherPore FluidMoisture Swelling.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Enter the following data in the Data table:
Strain
Volumetric moisture swelling strain, 
.
Saturation
Saturation, s. This value must lie in the range 
.
If you want to define anisotropic swelling, select Ratios from the Suboptions menu. See “Defining anisotropic swelling” for detailed instructions.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can include anisotropy in moisture swelling behavior by defining the ratios 
, 
, and 
such that two or more of the three ratios differ. The orientation of the moisture swelling strain directions depends on the user-specified local orientation (see “Orientations,” Section 2.2.5 of the Abaqus Analysis User's Guide).
To define anisotropic swelling:
Define moisture swelling behavior, as described in “Defining moisture swelling.”
From the Suboptions menu in the Edit Material dialog box, select Ratios.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define the anisotropy ratios as a function of temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables included in the definition of the anisotropy ratios.
In the Data table, enter the anisotropy ratios , , and . Enter values for temperature and field variables if applicable.
For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Click OK to return to the Edit Material dialog box.
Permeability is the relationship between the volumetric flow rate per unit area of a particular wetting liquid through a porous medium and the gradient of the effective fluid pressure. For more information, see “Permeability,” Section 26.6.2 of the Abaqus Analysis User's Guide.
You can use the Edit Material dialog box to define certain aspects of permeability. See the following sections for details:
You must specify permeability for a wetting liquid in Abaqus/Standard for an effective stress/wetting liquid diffusion analysis. For more information, see “Permeability,” Section 26.6.2 of the Abaqus Analysis User's Guide.
To define permeability in an Abaqus/Standard analysis:
From the menu bar in the Edit Material dialog box, select OtherPore FluidPermeability.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Type field, and specify the directional dependence of the permeability.
Enter a value for Specific weight of wetting liquid.
Toggle on Use temperature-dependent data to define permeability as a function of temperature.
A column labeled Temp appears in the Data table.
Enter the applicable data in the Data table:
k
Isotropic permeability of the fully saturated medium, k. (Units of LT–1.)
k11, k22, and k33
Three values for orthotropic permeability, 
, 
, and 
. (Units of LT–1.)
k11, k12, k22, k13, k23, and k33
Six values for anisotropic permeability, , 
, , 
, 
, and . (Units of LT–1.)
Void Ratio
Void ratio, e.
Temp
Temperature.
If you want to define the dependence of permeability on saturation, select Saturation Dependence from the Suboptions menu. See “Defining the saturation dependence of permeability” for detailed instructions.
If you want to define the dependence of permeability on velocity, select Velocity Dependence from the Suboptions menu. See “Defining the velocity dependence of permeability” for detailed instructions.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can define the dependence of permeability, 
, on saturation, s, by specifying 
. Abaqus/Standard assumes by default that 
for 
; 
for 
. The tabular definition of 
must specify for .
For more information, see “Permeability,” Section 26.6.2 of the Abaqus Analysis User's Guide.
To define saturation dependence:
Define permeability, as described in “Defining permeability in an Abaqus/Standard analysis.”
From the Suboptions menu in the Edit Material dialog box, select Saturation Dependence.
A Suboption Editor appears.
Enter the following data in the Data table:
k_s
The dependence of permeability on saturation of the wetting liquid.
Saturation
The fluid saturation (
for a fully saturated medium; 
for a completely dry medium).
Click OK to return to the Edit Material dialog box.
Permeability is defined, in general, by Forchheimer's law, which accounts for changes in permeability as a function of fluid flow velocity. The Suboption Editor allows you define the velocity coefficient as a function of the void ratio of the material. For more information, see “Permeability,” Section 26.6.2 of the Abaqus Analysis User's Guide.
To define saturation dependence:
Define permeability, as described in “Defining permeability in an Abaqus/Standard analysis.”
From the Suboptions menu in the Edit Material dialog box, select Velocity Dependence.
A Suboption Editor appears.
Enter the following data in the Data table:
Beta
Velocity coefficient, 
.
Void ratio
Void ratio, e.
Click OK to return to the Edit Material dialog box.
Permeability in Abaqus/CFD must be specified for porous media flows and can be isotropic with dependence on porosity. For more information, see “Permeability,” Section 26.6.2 of the Abaqus Analysis User's Guide.
To define permeability in an Abaqus/CFD analysis:
From the menu bar in the Edit Material dialog box, select OtherPore FluidPermeability.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Type field, and select Isotropic (CFD).
Specify a value for the Inertial drag coefficient. Set this parameter proportional to the value of the inertial (quadratic or form) drag in the porous medium. The default value is 0.142887.
Enter the applicable data in the Data table:
K
Isotropic permeability of the fully saturated medium, K. (Units of L2.)
Porosity
Porosity, 
.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
Permeability in Abaqus/CFD must be specified for porous media flows and can be specified through the Carman-Kozeny permeability-porosity relation. For more information, see “Permeability,” Section 26.6.2 of the Abaqus Analysis User's Guide.
To define permeability based on the Carman-Kozeny relation:
From the menu bar in the Edit Material dialog box, select OtherPore FluidPermeability.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Type field, and select Carman-Kozeny.
Specify a value for the Inertial drag coefficient. Set this parameter proportional to the value of the inertial (quadratic or form) drag in the porous medium. The default value is 0.142887.
In the Kozeny Constant field, enter a value for the Carman-Kozeny constant.
In the Pore Particle Radius field, enter a value for the pore-particle radius. For a fibrous medium, the radius is equal to the characteristic fiber radius.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can use the Edit Material dialog box to define thermal expansion for the pore fluid in a porous medium. For more information, see “Thermal expansion,” Section 26.1.2 of the Abaqus Analysis User's Guide.
To define pore fluid expansion:
From the menu bar in the Edit Material dialog box, select OtherPore FluidPore Fluid Expansion.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
In the Reference temperature field, enter a value for reference temperature if the coefficient of thermal expansion is a function of temperature or field variables
Toggle on Use temperature-dependent data to define the expansion coefficient as a function of temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the expansion coefficient depends.
Enter the following data in the Data table:
Expansion Coeff
Thermal expansion coefficient, 
. (Units of 
–1.)
Temp
Temperature.
Field n
Predefined field variables.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can define the bulk moduli of solid grains and a permeating fluid such that their compressibility can be considered in the analysis of a porous medium. For more information, see “Porous bulk moduli,” Section 26.6.3 of the Abaqus Analysis User's Guide.
To define porous bulk moduli:
From the menu bar in the Edit Material dialog box, select OtherPore FluidPorous Bulk Moduli.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Toggle on Use temperature-dependent data to define the bulk moduli as a function of temperature.
A column labeled Temp appears in the Data table.
Enter the following data in the Data table:
Bulk mod of grains
Bulk modulus of solid grains. (Units of FL–2.)
Bulk mod of fluids
Bulk modulus of permeating fluid. (Units of FL–2.)
Temp
Temperature.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can define absorption and exsorption behaviors of a partially saturated porous medium in the analysis of coupled wetting liquid flow and porous medium stress. For more information, see “Sorption,” Section 26.6.4 of the Abaqus Analysis User's Guide.
To define sorption:
From the menu bar in the Edit Material dialog box, select OtherPore FluidSorption.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Display the Absorption tabbed page.
Click the arrow to the right of the Law field, and specify how you want to define absorption behavior:
Select Log to define absorption behavior by the analytical logarithmic form.
Select Tabular to define absorption behavior in tabulated form.
If you selected Log in the previous step, enter the following data in the Data table:
A
A. This value must be positive. (Dimensionless.)
B
B. This value must be positive. (Units of L2F–1.)
s0
. This value must lie in the range 
. The default is 0.01.
s1
. This value must lie in the range . The default is 0.01 plus a very small positive number (since cannot be equal to ).
If you selected Tabular in Step 3, enter the following data in the Data table:
Pore Pressure
Pore pressure, 
, with the condition 
. (Units of FL–2.)
Saturation
Saturation, s. This value must lie in the range 
If you want to include exsorption behavior in the sorption definition, display the Exsorption tabbed page, and toggle on Include exsorption. Otherwise, skip to Step 12.
Click the arrow to the right of the Law field, and specify how you want to define exsorption behavior:
Select Log to define exsorption behavior by the analytical logarithmic form.
Select Tabular to define exsorption behavior in tabulated form.
Toggle on Include scanning to define the behavior between absorption and exsorption by a scanning line of constant slope, 
. This slope should be larger than the slope of any segment of the absorption or exsorption behaviors.
If you define sorption behavior without specifying a scanning line slope, Abaqus uses a slope of 1.05 times the largest value of 
provided in the absorption and exsorption behavior definitions.
If you toggled on Include scanning, enter a value for the slope of the scanning line in the Slope field.
If you selected Log in Step 7, enter the following data in the Data table:
A
A. This value must be positive. (Dimensionless.)
B
B. This value must be positive. (Units of L2F–1.)
s0
. This value must lie in the range . The default is 0.01.
s1
. This value must lie in the range . The default is 0.01 plus a very small positive number (since cannot be equal to ).
If you selected Tabular in Step 7, enter the following data in the Data table:
Pore Pressure
Pore pressure, , with the condition . (Units of FL–2.)
Saturation
Saturation, s. This value must lie in the range
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can model normal flow across gap surfaces by defining a fluid leakoff coefficient for the pore fluid material. This coefficient defines a pressure-flow relationship between the cohesive element's middle nodes and their adjacent surface nodes. The fluid leakoff coefficients can be interpreted as the permeability of a finite layer of material on the cohesive element surfaces. See the following sections for more information:
To define fluid leakoff coefficients
From the menu bar in the Edit Material dialog box, select OtherPore FluidFluid Leakoff.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Type field, and specify how you want to define the fluid leakoff coefficients:
Select Coefficients to enter the coefficients directly in the Edit Material dialog box.
Select User to define the coefficients in user subroutine UFLUIDLEAKOFF. If you select this option, skip to Step 6.
Toggle on Use temperature-dependent data to define the fluid leakoff coefficients as a function of temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the fluid leakoff coefficients depend.
Enter the following data in the Data table:
Top Coefficient
Fluid leak-off coefficient at the top element surface.
Bottom Coefficient
Fluid leak-off coefficient at the bottom element surface.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).
You can use the Edit Material dialog box to define tangential flow constitutive parameters for pore pressure cohesive elements. For more information, see “Defining the constitutive response of fluid within the cohesive element gap,” Section 32.5.7 of the Abaqus Analysis User's Guide.
To define tangential flow parameters:
From the menu bar in the Edit Material dialog box, select OtherPore FluidGap Flow.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.7.1.)
Click the arrow to the right of the Type field, and specify how you want to define the flow parameters:
Select Newtonian to define the viscosity for a Newtonian fluid.
Select Power law to define the consistency and exponent for a power law fluid.
Toggle on Use temperature-dependent data to define the flow parameters as a function of temperature.
A column labeled Temp appears in the Data table.
Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the flow parameters depend.
If you selected Newtonian in Step 2, you can toggle on Maximum permeability to enter the maximum permeability value that Abaqus can use.
If you selected Newtonian in Step 2, enter the following data in the Data table:
Viscosity
Pore fluid viscosity, 
.
Temp
Temperature.
Field n
Predefined field variables.
If you selected Power law in Step 2, enter the following data in the Data table:
Consistency
Fluid consistency, K.
Exponent
Power law exponent, 
.
Temp
Temperature.
Field n
Predefined field variables.
Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see “Browsing and modifying material behaviors,” Section 12.7.2, for more information).