ProductsAbaqus/StandardAbaqus/CAE Typical applicationsSome of the more common coupled pore fluid diffusion/stress (and, optionally, thermal) analysis problems that can be analyzed with Abaqus/Standard are:
Flow through porous mediaA porous medium is modeled in Abaqus/Standard by a conventional approach that considers the medium as a multiphase material and adopts an effective stress principle to describe its behavior. The porous medium modeling provided considers the presence of two fluids in the medium. One is the “wetting liquid,” which is assumed to be relatively (but not entirely) incompressible. Often the other is a gas, which is relatively compressible. An example of such a system is soil containing ground water. When the medium is partially saturated, both fluids exist at a point; when it is fully saturated, the voids are completely filled with the wetting liquid. The elementary volume, , is made up of a volume of grains of solid material, ; a volume of voids, ; and a volume of wetting liquid, , that is free to move through the medium if driven. In some systems (for example, systems containing particles that absorb the wetting liquid and swell in the process) there may also be a significant volume of trapped wetting liquid, . The porous medium is modeled by attaching the finite element mesh to the solid phase; fluid can flow through this mesh. The mechanical part of the model is based on the effective stress principle defined in Effective stress principle for porous media. The model also uses a continuity equation for the mass of wetting fluid in a unit volume of the medium. This equation is described in Continuity statement for the wetting liquid phase in a porous medium. It is written with pore pressure (the average pressure in the wetting fluid at a point in the porous medium) as the basic variable (degree of freedom 8 at the nodes). The conjugate flux variable is the volumetric flow rate at the node, . The porous medium is partially saturated when the pore liquid pressure, , is negative. Coupled flow and heat transfer through porous mediaOptionally, heat transfer due to conduction in the soil skeleton and pore fluid, as well as convection in the pore fluid, can also be modeled. This capability represents an enhancement to the basic pore fluid flow capabilities discussed in the earlier paragraphs and requires the use of coupled temperature–pore pressure elements that have temperature as an additional degree of freedom (degree of freedom 11 at the nodes) in addition to the pore pressure and the displacement components. When you use the coupled temperature–pore pressure elements, Abaqus solves the heat transfer equation in addition to and in a fully coupled manner with the continuity equation and the mechanical equilibrium equations. Only linear brick, first-order axisymmetric, and second-order modified tetrahedrons are available for modeling coupled heat transfer with pore fluid flow and mechanical deformation. Total and excess pore fluid pressureThe coupled pore fluid diffusion/stress analysis capability can provide solutions either in terms of total or “excess” pore fluid pressure. The excess pore fluid pressure at a point is the pore fluid pressure in excess of the hydrostatic pressure required to support the weight of pore fluid above the elevation of the material point. The difference between total and excess pore pressure is relevant only for cases in which gravitational loading is important; for example, when the loading provided by the hydrostatic pressure in the pore fluid is large or when effects like “wicking” (transient capillary suction of liquid into a dry column) are being studied. Total pore pressure solutions are provided when the gravity distributed load is used to define the gravity load on the model. Excess pore pressure solutions are provided in all other cases; for example, when gravity loading is defined with body force distributed loads. Steady-state analysisSteady-state coupled pore pressure/effective stress analysis assumes that there are no transient effects in the wetting liquid continuity equation; that is, the steady-state solution corresponds to constant wetting liquid velocities and constant volume of wetting liquid per unit volume in the continuum. Thus, for example, thermal expansion of the liquid phase has no effect on the steady-state solution: it is a transient effect. Therefore, the time scale chosen during steady-state analysis is relevant only to rate effects in the constitutive model used for the porous medium (excluding creep and viscoelasticity, which are disabled in steady-state analysis). Mechanical loads and boundary conditions can be changed gradually over the step by referring to an amplitude curve to accommodate possible geometric nonlinearities in the response. The steady-state coupled equations are strongly unsymmetric; therefore, the unsymmetric matrix solution and storage scheme is used automatically for steady-state analysis steps (see Defining an analysis). If heat transfer is modeled using the coupled temperature–pore pressure elements, the steady-state solution neglects all transient effects in the heat transfer equation and provides only the steady-state temperature distribution. Input File Usage SOILS Abaqus/CAE Usage Step module: Create Step: General: Soils: Basic: Pore fluid response: Steady state IncrementationYou can specify a fixed time increment size in a coupled pore fluid diffusion/stress analysis, or Abaqus/Standard can select the time increment size automatically. Automatic incrementation is recommended because the time increments in a typical diffusion analysis can increase by several orders of magnitude during the simulation. If you do not activate automatic incrementation, fixed time increments will be used. Input File Usage Use the following option to activate automatic incrementation in steady-state analysis: SOILS, UTOL=any arbitrary nonzero value The solution does not depend on the value specified for UTOL; this value is simply a flag for automatic incrementation. Abaqus/CAE Usage Step module: Create Step: General: Soils: Basic: Pore fluid response: Steady state; Incrementation: Type: Automatic Transient analysisIn a transient coupled pore pressure/effective stress analysis the backward difference operator is used to integrate the continuity equation and the heat transfer equation (if heat transfer is modeled): this operator provides unconditional stability so that the only concern with respect to time integration is accuracy. You can provide the time increments, or they can be selected automatically. The coupled partially saturated flow equations are strongly unsymmetric, so the unsymmetric solver is used automatically if you request partially saturated analysis (by including absorption/exsorption behavior in the material definition). The unsymmetric solver is also activated automatically when gravity distributed loading is used during a soils consolidation analysis. For fully saturated flow analyses in which finite-sliding coupled pore pressure-displacement contact is modeled using contact pairs, certain contributions to the model's stiffness matrix are unsymmetric. Using the unsymmetric solver can sometimes improve convergence in such cases since Abaqus does not automatically do so. For fully saturated flow analyses in which heat transfer is also modeled, the contributions to the model's stiffness matrix arising from convective heat transfer due to pore fluid flow are unsymmetric. Using the unsymmetric solver can sometimes improve convergence in such cases since Abaqus does not automatically do so. Spurious oscillations due to small time incrementsThe integration procedure used in Abaqus/Standard for consolidation analysis introduces a relationship between the minimum usable time increment and the element size, as shown below for fully saturated and partially saturated flows. If time increments smaller than these values are used, spurious oscillations may appear in the solution (except for partially saturated cases when linear elements or modified triangular elements are used; in these cases Abaqus/Standard uses a special integration scheme for the wetting liquid storage term to avoid the problem). These nonphysical oscillations may cause problems if pressure-sensitive plasticity is used to model the porous medium and may lead to convergence difficulties in partially saturated analyses. If the problem requires analysis with smaller time increments than the relationships given below allow, a finer mesh is required. Generally there is no upper limit on the time step except accuracy, since the integration procedure is unconditionally stable unless nonlinearities cause convergence problems. Fully saturated flowA simple guideline that can be used for the minimum usable time increment in the case of fully saturated flow is where
Partially saturated flowIn partially saturated flow cases the corresponding guideline for the minimum time increment is where
Fixed incrementationIf you choose fixed time incrementation, fixed time increments equal to the size of the user-specified initial time increment, , will be used. Fixed incrementation is not generally recommended because the time increments in a typical diffusion analysis can increase over several orders of magnitude during the simulation; automatic incrementation is usually a better choice. Input File Usage SOILS, CONSOLIDATION Abaqus/CAE Usage Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation; Incrementation: Type: Fixed, Increment size: Automatic incrementationIf you choose automatic time incrementation, you must specify two (three if heat transfer is also modeled) tolerance parameters. The accuracy of the time integration of the flow continuity equations is governed by the maximum wetting liquid pore pressure change, , allowed in an increment. Abaqus/Standard restricts the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment in the analysis. If heat transfer is modeled, the accuracy of time integration is also governed by the maximum temperature change, , allowed in an increment. Abaqus/Standard restricts the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis. The accuracy of the integration of the time-dependent (creep) material behavior is governed by the maximum strain rate change allowed at any point during an increment, , as described in Rate-dependent plasticity: creep and swelling. Input File Usage If heat transfer is not modeled: SOILS, CONSOLIDATION, UTOL=, , CETOL=errtol If heat transfer is modeled: SOILS, CONSOLIDATION, UTOL=, DELTMX=, CETOL=errtol Abaqus/CAE Usage Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation; Incrementation: Type: Automatic, Max. pore pressure change per increment: , Creep/swelling/viscoelastic strain error tolerance: errtol Specifying the maximum temperature change per increment is not supported in Abaqus/CAE. Ending a transient analysisTransient soils analysis can be terminated by completing a specified time period, or it can be continued until steady-state conditions are reached. By default, the analysis will end when the given time period has been completed. Alternatively, you can specify that the analysis will end when steady state is reached or the time period ends, whichever comes first. When heat transfer is not modeled, steady state is defined by a maximum permitted rate of change of pore pressure with time: when all pore pressures are changing at less than the user-defined rate, the analysis terminates. However, with heat transfer included, the analysis terminates only when both the pore pressure and temperature are changing at less than the user-defined rates. Input File Usage Use the following option to end the analysis when the time period is reached: SOILS, CONSOLIDATION, END=PERIOD (default) Use the following option to end the analysis based on the pore pressure and, if heat transfer is modeled, temperature change rate: SOILS, CONSOLIDATION, END=SS Abaqus/CAE Usage Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation; Incrementation: End step when pore pressure change rate is less than If heat transfer is modeled, directly specifying the temperature change rate to define steady state is not supported in Abaqus/CAE. Neglecting creep during a transient analysisYou can specify that creep or viscoelastic response should be neglected during a consolidation analysis, even if creep or viscoelastic material properties have been defined. Input File Usage SOILS, CONSOLIDATION, CREEP=NONE Abaqus/CAE Usage Step module: Create Step: General: Soils: Basic: Pore fluid response: Transient consolidation, toggle off Include creep/swelling/viscoelastic behavior Unstable problemsSome types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers the option to stabilize this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in Automatic stabilization of unstable problems. Optional modeling of coupled heat transferWhen 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 some steps in the analysis. This feature may be helpful in reducing computation time during certain phases in the analysis when heat transfer is not an important part of the overall physics of the problem. Input File Usage Use the following option either during a transient or a steady-state procedure to suppress heat transfer modeling: SOILS, CONSOLIDATION, HEAT=NO Abaqus/CAE Usage Switching off the heat transfer part of the physics is not supported in Abaqus/CAE. UnitsIn coupled problems where two or more different fields are being solved, you must be careful when choosing the units of the problem. If the choice of units is such that the numbers generated by the equations for the different fields differ by many orders of magnitude, the precision on some computers may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid badly conditioned matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress equilibrium equations and the pore flow continuity equations. Initial conditionsInitial conditions can be applied as defined in Initial conditions in Abaqus/Standard and Abaqus/Explicit. Defining initial pore fluid pressuresInitial values of pore fluid pressures, , can be defined at the nodes. Input File Usage INITIAL CONDITIONS, TYPE=PORE PRESSURE Abaqus/CAE Usage Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Pore pressure for the Types for Selected Step Defining initial void ratiosInitial values of the void ratio, e, can be given at the nodes. The void ratio is defined as the ratio of the volume of voids to the volume of solid material (see Effective stress principle for porous media). The evolution of void ratio is governed by the deformation of the different phases of the material, as discussed in detail in Constitutive behavior in a porous medium. Input File Usage INITIAL CONDITIONS, TYPE=RATIO Abaqus/CAE Usage Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Void ratio for the Types for Selected Step Defining initial saturationInitial saturation values, s, can be given at the nodes. Saturation is defined as the ratio of wetting fluid volume to void volume (see Effective stress principle for porous media). Input File Usage INITIAL CONDITIONS, TYPE=SATURATION Abaqus/CAE Usage Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Saturation for the Types for Selected Step Defining initial stressesAn initial (effective) stress field can be specified (see Initial conditions in Abaqus/Standard and Abaqus/Explicit). 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 and usually includes both horizontal and vertical components. It is important to establish these initial conditions correctly so that the problem begins from an equilibrium state. The geostatic procedure can be used to verify that the user-defined initial stresses are indeed in equilibrium with the given geostatic loads and boundary conditions (see Geostatic stress state). Input File Usage Use one of the following options: INITIAL CONDITIONS, TYPE=STRESS INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Abaqus/CAE Usage Load module: Create Predefined Field: Step: Initial: choose Mechanical for the Category and Stress or Geostatic stress for the Types for Selected Step Defining initial temperatureInitial temperature values can be defined at the nodes. Input File Usage INITIAL CONDITIONS, TYPE=TEMPERATURE Abaqus/CAE Usage Load module: Create Predefined Field: Step: Initial: choose Other for the Category and Temperature for the Types for Selected Step Boundary conditionsBoundary 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). In addition, boundary conditions can also be applied to temperature degree of freedom 11 if heat transfer is modeled using coupled temperature–pore pressure elements. During the analysis prescribed boundary conditions can be varied by referring to an amplitude curve (Amplitude Curves). If no amplitude reference is given, the default variation of a boundary condition in a coupled pore fluid diffusion/stress analysis step is as defined in Defining an analysis. If the pore pressure is prescribed with a boundary condition, fluid is assumed to enter and leave through the node as needed to maintain the prescribed pressure. Likewise, if the temperature is prescribed with a boundary condition, heat is assumed to enter and leave through the node as needed to maintain the prescribed temperature. LoadsThe following loading types can be prescribed in a coupled pore fluid diffusion/stress analysis:
If heat transfer is modeled, the following types of thermal loading can also be prescribed (Thermal loads). These loads are not supported in Abaqus/CAE during a coupled thermal pore pressure/stress analysis.
Predefined fieldsThe following predefined fields can be prescribed, as described in Predefined Fields:
Material optionsAny of the mechanical constitutive models available in Abaqus/Standard can be used to model the porous material. In problems formulated in terms of total pore pressure, you must include the density of the dry material in the material definition (see Density). You can use a permeability material property to define the specific weight of the wetting liquid, ; the permeability, , and its dependence on the void ratio, e, and saturation, ; and the flow velocity, (see Permeability). You can define the compressibility of the solid grains and of the permeating fluid in both fully and partially saturated flow problems (see Elastic behavior of porous materials). If you do not specify the porous bulk moduli, the materials are assumed to be fully incompressible. For partially saturated flow you must define the porous medium's absorption/exsorption behavior (see Sorption). Gel swelling (Swelling gel) and volumetric moisture swelling of the solid skeleton (Moisture swelling) can be included in partially saturated cases. These effects are usually associated with modeling of moisture migration in polymeric systems rather than with geotechnical systems. Thermal properties if heat transfer is modeledIn problems that model heat transfer, the thermal conductivity for either the solid material or the permeating fluid, or more commonly for both phases, must be defined. Only isotropic conductivity can be specified for the pore fluid. The specific heat and density of the phases must also be defined for transient heat transfer problems. Latent heat for the phases can be defined if changes in internal energy due to phase changes are important. See About thermal properties for details on defining thermal properties in Abaqus. Examples of problems that model fully coupled heat transfer along with pore fluid diffusion and mechanical deformation can be found in Consolidation around a cylindrical heat source and Permafrost thawing–pipeline interaction. The thermal properties can be defined separately for the solid material and the permeating fluid. Input File Usage To define the conductivity, specific heat, density, and latent heat of the permeating fluid, use the following options: CONDUCTIVITY, TYPE=ISO, PORE FLUID SPECIFIC HEAT, PORE FLUID LATENT HEAT, PORE FLUID DENSITY, PORE FLUID To define the conductivity, specific heat, density, and latent heat of the solid material, use the following options: EXPANSION, TYPE=ISO or ORTHO or ANISO SPECIFIC HEAT DENSITY LATENT HEAT Abaqus/CAE Usage Defining the thermal properties and the density of the permeating fluid is not supported in Abaqus/CAE. To define the conductivity, specific heat, density, and latent heat of the solid material, use the following options: Property module: material editor: Type: Isotropic: Thermal expansionThermal expansion can be defined separately for the solid material and for the permeating fluid. In such a case you should repeat the expansion material property, with the necessary parameters, to define the different thermal expansion effects (see Thermal expansion). Thermal expansion will be active only in a consolidation (transient) analysis. Input File Usage To define the thermal expansion of the permeating fluid: EXPANSION, TYPE=ISO, PORE FLUID To define the thermal expansion of the solid material: EXPANSION, TYPE=ISO or ORTHO or ANISO Abaqus/CAE Usage To define the thermal expansion of the permeating fluid: Property module: material editor: To define the thermal expansion of the solid material: Property module: material editor: ElementsThe analysis of flow through porous media in Abaqus/Standard is available for plane strain, axisymmetric, and three-dimensional problems. The modeling of coupled heat transfer effects is available only for axisymmetric and three-dimensional problems. Continuum pore pressure elements are provided for modeling fluid flow through a deforming porous medium in a coupled pore fluid diffusion/stress analysis. These elements have pore pressure degree of freedom 8 in addition to displacement degrees of freedom 1–3. Heat transfer through the porous medium can also be modeled using continuum coupled temperature–pore pressure elements. These elements have temperature degree of freedom 11 in addition to pore pressure degree of freedom 8 and displacement degrees of freedom 1–3. Stress/displacement elements can be used in parts of the model without pore fluid flow. See Choosing the appropriate element for an analysis type for more information. OutputThe 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:
If heat transfer is modeled, the following element output variables associated with heat transfer are also available:
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:
If heat transfer is modeled, the following nodal output variables associated with heat transfer are also available:
All of the output variable identifiers are outlined in Abaqus/Standard output variable identifiers. Input file templateHEADING … *********************************** ** ** Material definition ** *********************************** MATERIAL, NAME=soil Data lines to define mechanical properties of the solid material … EXPANSION Data lines to define the thermal expansion coefficient of the solid grains EXPANSION, TYPE=ISO, PORE FLUID Data lines to define the thermal expansion coefficient of the permeating fluid PERMEABILITY, SPECIFIC= Data lines to define permeability, , as a function of the void ratio, e PERMEABILITY, TYPE=SATURATION Data lines to define the dependence of permeability on saturation, PERMEABILITY, TYPE=VELOCITY Data lines to define the velocity coefficient, POROUS BULK MODULI Data line to define the bulk moduli of the solid grains and the permeating fluid SORPTION, TYPE=ABSORPTION Data lines to define absorption behavior SORPTION, TYPE=EXSORPTION Data lines to define exsorption behavior SORPTION, TYPE=SCANNING Data lines to define scanning behavior (between absorption and exsorption) GEL Data line to define gel behavior in partially saturated flow MOISTURE SWELLING Data lines to define moisture swelling strain as a function of saturation in partially saturated flow 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 SPECIFIC HEAT,PORE FLUID Data lines to define specific heat of the permeating fluid if transient heat transfer is modeled DENSITY Data lines to define density of the solid grains if transient heat transfer is modeled DENSITY,PORE FLUID Data lines to define density of the permeating fluid if transient heat transfer is modeled 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 … *********************************** ** ** Boundary conditions and initial conditions ** *********************************** BOUNDARY Data lines to specify zero-valued boundary conditions INITIAL CONDITIONS, TYPE=STRESS, GEOSTATIC Data lines to specify initial stresses 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 saturation AMPLITUDE, NAME=name Data lines to define amplitude variations *********************************** ** ** Step 1: Optional step to ensure an equilibrium ** geostatic stress field ** *********************************** STEP GEOSTATIC CLOAD and/or DLOAD and/or TEMPERATURE and/or FIELD 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 *********************************** ** ** Step 2: Coupled pore diffusion/stress analysis step ** *********************************** STEP (,NLGEOM) ** Use NLGEOM to include geometric nonlinearities SOILS Data line to define incrementation 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 FILM Data lines referring to film property table if heat transfer is modeled BOUNDARY Data lines to specify displacements, pore pressures, or temperatures END STEP |