Products: Abaqus/Standard Abaqus/CAE
A geostatic stress field procedure:
is used to verify that the initial geostatic stress field is in equilibrium with applied loads and boundary conditions and to iterate, if necessary, to obtain equilibrium;
accounts for pore pressure degrees of freedom when pore pressure elements are used, and accounts for temperature degrees of freedom when coupled temperature–pore pressure elements are used;
is usually the first step of a geotechnical analysis, followed by a coupled pore fluid diffusion/stress (with or without heat transfer) or static analysis procedure; and
can be linear or nonlinear.
The geostatic procedure is normally used as the first step of a geotechnical analysis; in such cases gravity loads are applied during this step. Ideally, the loads and initial stresses should exactly equilibrate and produce zero deformations. However, in complex problems it may be difficult to specify initial stresses and loads that equilibrate exactly.
Abaqus/Standard provides two procedures for establishing the initial equilibrium. The first procedure is applicable to problems for which the initial stress state is known at least approximately. The second, enhanced, procedure is also applicable for cases in which the initial stresses are not known; it is supported for only a limited number of elements and materials.
The geostatic procedure requires that the initial stresses are close to the equilibrium state; otherwise, the displacements corresponding to the equilibrium state might be large. Abaqus/Standard checks for equilibrium during the geostatic procedure and iterates, if needed, to obtain a stress state that equilibrates the prescribed boundary conditions and loads. This stress state, which is a modification of the stress field defined by the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1), is then used as the initial stress field in a subsequent static or coupled pore fluid diffusion/stress (with or without heat transfer) analysis.
If the stresses given as initial conditions are far from equilibrium under the geostatic loading and there is some nonlinearity in the problem definition, this iteration process may fail. Therefore, you should ensure that the initial stresses are reasonably close to equilibrium.
If the deformations produced during the geostatic step are significant compared to the deformations caused by subsequent loading, the definition of the initial state should be reexamined.
If heat transfer is modeled during the geostatic step through the use of coupled temperature–pore pressure elements, the initial temperature field and thermal loads, if specified, must be such that the system is relatively close to a state of thermal equilibrium. Steady-state heat transfer is assumed during a geostatic step.
| Input File Usage: | *GEOSTATIC |
| Abaqus/CAE Usage: | Step module: Create Step: General: Geostatic |
To obtain equilibrium in cases when the initial stress state is unknown or is known only approximately, you can invoke an enhanced procedure. Abaqus automatically computes the equilibrium corresponding to the initial loads and the initial configuration, allowing only small displacements within user-specified tolerances. (The default tolerance is 
.) The procedure is available with a limited number of elements and materials and is intended to be used in analyses in which the material response is primarily elastic; that is, inelastic deformations are small.
The procedure is supported for both geometrically linear and geometrically nonlinear analyses. However, in general, the performance in the geometrically linear case will be better. Therefore, it might be advantageous to obtain the initial equilibrium in a geometrically linear step, even though a geometrically nonlinear analysis is performed in subsequent steps.
| Input File Usage: | Use the following option to invoke the enhanced procedure: |
*GEOSTATIC, UTOL=displacement tolerance |
| Abaqus/CAE Usage: | Step module: Create Step: General: Geostatic: Incrementation tabbed page: Automatic: Max. displacement change |
The following limitations apply to the enhanced procedure:
It is supported only for a limited number of elements (see “Elements” below) and materials (see “Material options” below). When the procedure is used with nonsupported elements or material models, Abaqus issues a warning message. In this case it is the user's responsibility to ensure that the displacement tolerances are larger than the displacements in the analysis; otherwise, convergence problems may occur.
It can be used in a restart analysis only if it had been used in the previous analysis.
When coupled temperature–pore pressure elements are used, heat transfer is modeled in these elements by default. However, you may optionally choose to switch off heat transfer within these elements during a geostatic step. This feature may be helpful in reducing computation time if temperature and associated heat flow effects are not important.
| Input File Usage: | Use the following option to suppress heat transfer modeling: |
*GEOSTATIC, HEAT=NO |
| Abaqus/CAE Usage: | Switching off the heat transfer part of the physics is not supported in Abaqus/CAE. |
Most geotechnical problems begin from a geostatic state, which is a steady-state equilibrium configuration of the undisturbed soil or rock body under geostatic loading. The equilibrium state usually includes both horizontal and vertical stress components. It is important to establish these initial conditions correctly so that the problem begins from an equilibrium state. Since such problems often involve fully or partially saturated flow, the initial void ratio of the porous medium, 
, the initial pore pressure, 
, and the initial effective stress must all be defined.
If the magnitude and direction of the gravitational loading are defined by using the gravity distributed load type, a total, rather than excess, pore pressure solution is used (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). This discussion is based on the total pore pressure formulation.
The z-axis points vertically in this discussion, and atmospheric pressure is neglected. We assume that the pore fluid is in hydrostatic equilibrium during the geostatic procedure so that
is the user-defined specific weight of the pore fluid (see “Permeability,” Section 26.6.2). (The pore fluid is not in hydrostatic equilibrium if there is significant steady-state flow of pore fluid through the porous medium: in that case a steady-state coupled pore fluid diffusion/stress analysis must be performed to establish the initial conditions for any subsequent transient calculations—see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1.) If we also take to be independent of z (which is usually the case, since the fluid is almost incompressible), this equation can be integrated to define
is the height of the phreatic surface, at which 
and above which 
and the pore fluid is only partially saturated.We usually assume that there are no significant shear stresses 
, 
. Then, equilibrium in the vertical direction is
is the dry density of the porous solid material (the dry mass per unit volume), g is the gravitational acceleration, 
is the initial porosity of the material, and s is the saturation, 
(see “Permeability,” Section 26.6.2). Since porosity is the ratio of pore volume to total volume and the void ratio is the ratio of pore volume to solids volume, is defined from the initial void ratio by
Abaqus/Standard requires that the initial value of the effective stress, 
, be given as an initial condition (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Effective stress is defined from the total stress, 
, by
is a unit matrix. Combining this definition with the equilibrium statement in the z-direction and hydrostatic equilibrium in the pore fluid gives
is independent of z. 
is the position of the surface that separates the dry soil from the partially saturated soil. The soil is assumed to be dry (
) for 
, and it is assumed to be partially saturated for 
and fully saturated for 
.In many cases s is constant. For example, in fully saturated flow 
everywhere below the phreatic surface. If we further assume that the initial porosity, , and the dry density of the porous medium, , are also constant, the above equation is readily integrated to give
is the position of the surface of the porous medium, 
.In more complicated cases where s, , and/or vary with height, the equation must be integrated in the vertical direction to define the initial values of 
.
In many geotechnical applications there is also horizontal stress, typically caused by tectonic action. If the pore fluid is under hydrostatic equilibrium and 
, equilibrium in the horizontal directions requires that the horizontal components of effective stress do not vary with horizontal position: 
only, where 
is any horizontal component of effective stress.
The initial effective geostatic stress field, , is given by defining initial stress conditions. Unless the enhanced procedure is used, the initial state of stress must be close to being in equilibrium with the applied loads and boundary conditions. See “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.
You can specify that the initial stresses vary only with elevation, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1. In this case the horizontal stress is typically assumed to be a fraction of the vertical stress: those fractions are defined in the x- and y-directions.
In problems involving partially or fully saturated porous media, initial pore fluid pressures, , void ratios, , and saturation values, s, must be given (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1).
In partially saturated cases the initial pore pressure and saturation values must lie on or between the absorption and exsorption curves (see “Sorption,” Section 26.6.4). A partially saturated problem is illustrated in “Wicking in a partially saturated porous medium,” Section 1.9.3 of the Abaqus Benchmarks Guide.
You may also specify initial temperatures in the model if heat transfer is modeled during the geostatic procedure.
Boundary conditions can be applied to displacement degrees of freedom 1–6 and to pore pressure degree of freedom 8 (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1). If coupled temperature–pore pressure elements are used, boundary conditions on temperature degree of freedom 11 can also be applied to nodes belonging to these elements. If the enhanced procedure is used and nonzero boundary conditions are applied, it is the user's responsibility to ensure that the displacements corresponding to the tolerances specified are larger than the displacements in the analysis; otherwise, the displacements at the nonzero boundary nodes will be reset to zero with the tolerances specified.
The boundary conditions should be in equilibrium with the initial stresses and applied loads. If the horizontal stress is nonzero, horizontal equilibrium must be maintained by fixing the boundary conditions on any nonhorizontal edges of the finite element model in the horizontal direction or by using infinite elements (“Infinite elements,” Section 28.3.1). If heat transfer is modeled, the temperature boundary conditions should be in equilibrium with the initial temperature field and applied thermal loads.
The following loading types can be prescribed in a geostatic stress field procedure:
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see “Concentrated loads,” Section 34.4.2.
Distributed pressure forces or body forces can also be applied; see “Distributed loads,” Section 34.4.3. The distributed load types available with particular elements are described in Part VI, “Elements.” The magnitude and direction of gravitational loading are defined by using the gravity or body force distributed load types.
Pore fluid flow is controlled as described in “Pore fluid flow,” Section 34.4.7.
If heat transfer is modeled, the following types of thermal loading can also be prescribed (“Thermal loads,” Section 34.4.4). These loads are not supported in Abaqus/CAE during a geostatic analysis.
Concentrated heat fluxes.
Body fluxes and distributed surface fluxes.
Convective film conditions and radiation conditions; film properties can be made a function of temperature.
The following predefined fields can be specified in a geostatic stress field procedure, as described in “Predefined fields,” Section 34.6.1:
For a geostatic analysis that does not model heat transfer and uses regular pore pressure elements, temperature is not a degree of freedom and nodal temperatures can be specified.
Predefined temperature fields are not allowed in a geostatic analysis that also models heat transfer. Boundary conditions should be used instead to specify temperatures, as described earlier.
The values of user-defined field variables can be specified; these values affect only field-variable-dependent material properties, if any.
Any of the mechanical constitutive models available in Abaqus/Standard can be used to model the porous solid material. However, the enhanced procedure can be used only with the elastic, porous elastic, extended Cam-clay plasticity, and Mohr-Coulomb plasticity models. Use of a nonsupported material model with this procedure may lead to poor convergence or no convergence if displacements are larger than the displacements corresponding to the tolerances specified. Abaqus will issue a warning message if the procedure is used with a nonsupported material model.
If a porous medium will be analyzed subsequent to the geostatic procedure, pore fluid flow quantities such as permeability and sorption should be defined (see “Pore fluid flow properties,” Section 26.6.1).
If heat transfer is modeled, thermal properties such as conductivity, specific heat, and density should be defined for both the solid and the pore fluid phases (see “Thermal properties if heat transfer is modeled” in “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1, for details on how to specify separate thermal properties for the two phases).
Any of the stress/displacement elements in Abaqus/Standard can be used in a geostatic procedure. Continuum pore pressure elements can also be used for modeling fluid in a deforming porous medium. These elements have pore pressure degree of freedom 8 in addition to displacement degrees of freedom 1–3. However, the enhanced procedure can be used only with continuum and cohesive elements with pore pressure degrees of freedom and the corresponding stress/displacements elements. Use of nonsupported elements with this procedure may lead to poor convergence or no convergence if displacements are larger than the displacements corresponding to the tolerances specified. Abaqus will issue a warning message if the procedure is used with a nonsupported element.
Continuum elements that couple temperature, pore pressure, and displacement can be used if heat transfer needs to be modeled. These elements have temperature degree of freedom 11 in addition to pore pressure degree of freedom 8 and displacement degrees of freedom 1–3. See “Choosing the appropriate element for an analysis type,” Section 27.1.3, for more information.
The element output available for a coupled pore fluid diffusion/stress analysis includes the usual mechanical quantities such as (effective) stress; strain; energies; and the values of state, field, and user-defined variables. In addition, the following quantities associated with pore fluid flow are available:
VOIDR | Void ratio, e. |
POR | Pore pressure, |
SAT | Saturation, s. |
GELVR | Gel volume ratio, |
FLUVR | Total fluid volume ratio, |
FLVEL | Magnitude and components of the pore fluid effective velocity vector, |
FLVELM | Magnitude, |
FLVELn | Component n of the pore fluid effective velocity vector (n=1, 2, 3). |
If heat transfer is modeled, the following element output variables associated with heat transfer are also available:
HFL | Magnitude and components of the heat flux vector. |
HFLn | Component n of the heat flux vector (n=1, 2, 3). |
HFLM | Magnitude of the heat flux vector. |
TEMP | Integration point temperatures. |
The nodal output available includes the usual mechanical quantities such as displacements, reaction forces, and coordinates. In addition, the following quantities associated with pore fluid flow are available:
POR | Pore pressure at a node. |
RVF | Reaction fluid volume flux due to prescribed pressure. This flux is the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pressure boundary condition. A positive value of RVF indicates fluid is entering the model. |
If heat transfer is modeled, the following nodal output variables associated with heat transfer are also available:
NT | Nodal point temperatures. |
RFL | Reaction flux values due to prescribed temperature. |
RFLn | Reaction flux value n at a node (n=11, 12, …). |
CFL | Concentrated flux values. |
CFLn | Concentrated flux value n at a node (n=11, 12, …). |
All of the output variable identifiers are outlined in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
*HEADING … *MATERIAL, NAME=mat1 Data lines to define mechanical properties of the solid material … *DENSITY Data lines to define the density of the dry material *PERMEABILITY, SPECIFIC=, as a function of the void ratio, e *CONDUCTIVITY Data lines to define thermal conductivity of the solid grains if heat transfer is modeled *CONDUCTIVITY,TYPE=ISO, PORE FLUID Data lines to define thermal conductivity of the permeating fluid if heat transfer is modeled *SPECIFIC HEAT Data lines to define specific heat of the solid grains if transient heat transfer is modeled in a subsequent step *SPECIFIC HEAT,PORE FLUID Data lines to define specific heat of the permeating fluid if transient heat transfer is modeled in a subsequent step *DENSITY Data lines to define density of the solid grains if transient heat transfer is modeled in a subsequent step *DENSITY,PORE FLUID Data lines to define density of the permeating fluid if transient heat transfer is modeled in a subsequent step *LATENT HEAT Data lines to define latent heat of the solid grains if phase change due to temperature change is modeled *LATENT HEAT,PORE FLUID Data lines to define latent heat of the permeating fluid if phase change due to temperature change is modeled … *INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Data lines to define the initial stress state *INITIAL CONDITIONS, TYPE=PORE PRESSURE Data lines to define initial values of pore fluid pressures *INITIAL CONDITIONS, TYPE=RATIO Data lines to define initial values of the void ratio *INITIAL CONDITIONS, TYPE=SATURATION Data lines to define initial saturation *INITIAL CONDITIONS, TYPE=TEMPERATURE Data lines to define initial temperature *BOUNDARY Data lines to define zero-valued boundary conditions ** *STEP *GEOSTATIC *CLOAD and/or *DLOAD and/or *DSLOAD Data lines to specify mechanical loading *FLOW and/or *SFLOW and/or *DFLOW and/or *DSFLOW Data lines to specify pore fluid flow *CFLUX and/or *DFLUX Data lines to define concentrated and/or distributed heat fluxes if heat transfer is modeled *BOUNDARY Data lines to specify displacements or pore pressures *END STEP
.
.
.
, of the pore fluid effective velocity vector.