김경종
14 KiB
Products: Abaqus/Standard Abaqus/CAE
References
• “Pore fluid flow properties,” Section 26.6.1
• “Material library: overview,” Section 21.1.1
• *MOISTURE SWELLING
• “Defining moisture swelling” in “Defining a fluid-filled porous material,” Section 12.12.3 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
Moisture swelling:
• defines the saturation-driven volumetric swelling of the solid skeleton of a porous medium in partially saturated flow conditions;
• can be used in the analysis of coupled wetting liquid flow and porous medium stress (see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1); and
• can be either isotropic or anisotropic.
Moisture swelling model
The moisture swelling model assumes that the volumetric swelling of the porous medium’s solid skeleton is a function of the saturation of the wetting liquid in partially saturated flow conditions. The porous medium is partially saturated when the pore liquid pressure, u _ { w } , is negative (see “Effective stress principle for porous media,” Section 2.8.1 of the Abaqus Theory Guide).
The swelling behavior is assumed to be reversible. The logarithmic measure of swelling strain is calculated with reference to the initial saturation so that
\varepsilon_ {i i} ^ {m s} = r _ {i i} \frac {1}{3} \left(\varepsilon^ {m s} (s) - \varepsilon^ {m s} (s ^ {I})\right), \quad (\mathrm{nosum} i)
where \varepsilon ^ { m s } ( s ) and \varepsilon ^ { m s } ( s ^ { I } ) are the volumetric swelling strains at the current and initial saturations. A typical curve is shown in Figure 26.6.6–1. The ratios r _ { 1 1 } , r _ { 2 2 } , and r _ { 3 3 } allow for anisotropic swelling as discussed below.
Defining volumetric swelling strain
Define the volumetric swelling strain, \varepsilon ^ { m s } , as a tabular function of the wetting liquid saturation, s. The swelling strain must be defined for the range 0 . 0 \leq s \leq 1 . 0 .
Input File Usage: \mathrm { * M O I S T U R E ~ S W E L L I N G }
line
| saturation | ε^ms(s^I) |
|---|---|
| 0.0 | ε^ms(s^I) |
| s^I | ε^ms(s^I) |
| s | ε^ms(s) |
| 1.0 | ε^ms(s) |
Figure 26.6.6–1 Typical volumetric moisture swelling versus saturation curve.
Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Moisture Swelling
Defining initial saturation values
You can define the initial saturation values as initial conditions. If no initial saturation values are given, the default is fully saturated conditions (saturation of 1.0). For partial saturation the initial saturation and pore fluid pressure must be consistent, in the sense that the pore fluid pressure must lie within the absorption and exsorption values for the initial saturation value (see “Permeability,” Section 26.6.2). If this is not the case, Abaqus/Standard will adjust the saturation value as needed to satisfy this requirement.
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 anisotropic swelling
Anisotropy can be included in moisture swelling behavior by defining the ratios r _ { 1 1 } , r _ { 2 2 } , and r _ { 3 3 } , such that two or more of the three ratios differ. If the ratios r _ { i i } are not specified, Abaqus/Standard assumes that the swelling is isotropic and that r _ { 1 1 } = r _ { 2 2 } = r _ { 3 3 } = 1 . 0 . The orientation of the moisture swelling strain directions depends on the user-specified local orientation (see “Orientations,” Section 2.2.5).
Input File Usage: Use both of the following options:
*MOISTURE SWELLING
*RATIOS
The *RATIOS option should immediately follow the *MOISTURE SWELLING option.
Abaqus/CAE Usage: Property module: material editor: Other→Pore Fluid→Moisture Swelling: Suboptions→Ratios
Elements
The moisture swelling model can be used only in elements that allow for pore pressure (see “Choosing the appropriate element for an analysis type,” Section 27.1.3).
26.7 User materials
• “User-defined mechanical material behavior,” Section 26.7.1
• “User-defined thermal material behavior,” Section 26.7.2
26.7.1 USER-DEFINED MECHANICAL MATERIAL BEHAVIOR
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “UMAT,” Section 1.1.44 of the Abaqus User Subroutines Reference Guide
• “VUMAT,” Section 1.2.22 of the Abaqus User Subroutines Reference Guide
• *USER MATERIAL
• *DEPVAR
• “Specifying solution-dependent state variables,” Section 12.8.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Defining constants for a user material,” Section 12.8.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
User-defined mechanical material behavior in Abaqus:
• is provided by means of an interface whereby any mechanical constitutive model can be added to the library;
• requires that a constitutive model (or a library of models) is programmed in user subroutine UMAT (Abaqus/Standard) or VUMAT (Abaqus/Explicit); and
• requires considerable effort and expertise: the feature is very general and powerful, but its use is not a routine exercise.
Stress components and strain increments
The subroutine interface has been implemented using Cauchy stress components (“true” stress). For soils problems “stress” should be interpreted as effective stress. The strain increments are defined by the symmetric part of the displacement increment gradient (equivalent to the time integral of the symmetric part of the velocity gradient).
The orientation of the stress and strain components in user subroutine UMAT depends on the use of local orientations (“Orientations,” Section 2.2.5).
In user subroutine VUMAT all strain measures are calculated with respect to the midincrement configuration. All tensor quantities are defined in the corotational coordinate system that rotates with the material point. To illustrate what this means in terms of stresses, consider the bar shown in Figure 26.7.1–1, which is stretched and rotated from its original configuration, , to its new position, A ^ { \prime } B ^ { \prime } . This deformation can be obtained in two stages; the bar is first stretched, as shown in Figure 26.7.1–2, and is then rotated by applying a rigid body rotation to it, as shown in Figure 26.7.1–3. The stress in the bar after it has been stretched is \sigma _ { 1 1 } , and this stress does not change during the rigid body rotation. The X ^ { \prime } Y ^ { \prime } coordinate system that rotates as a result of the rigid body rotation is the
text_image
Y B' α A' A B X
Figure 26.7.1–1 Stretched and rotated bar.
text_image
Y σ₁₁ ← σ₁₁ X
Figure 26.7.1–2 Stretching of bar.
text_image
Y Y' X' σ₁₁ α σ₁₁ X
Figure 26.7.1–3 Rigid body rotation of bar.
corotational coordinate system. The stress tensor and state variables are, therefore, computed directly and updated in user subroutine VUMAT using the strain tensor since all of these quantities are in the
corotational system; these quantities do not have to be rotated by the user subroutine as is sometimes required in user subroutine UMAT.
The elastic response predicted by a rate-form constitutive law depends on the objective stress rate employed. For example, the Green-Naghdi stress rate is used in VUMAT. However, the stress rate used for built-in material models may differ. For example, most material models used with solid (continuum) elements in Abaqus/Explicit employ the Jaumann stress rate. This difference in the formulation will cause significant differences in the results only if finite rotation of a material point is accompanied by finite shear. For a discussion of the objective stress rates used in Abaqus, see “Stress rates,” Section 1.5.3 of the Abaqus Theory Guide.
Material constants
Any material constants that are needed in user subroutine UMAT or VUMAT must be specified as part of a user-defined material behavior definition. Any other mechanical material behaviors included in the same material definition (except thermal expansion and, in Abaqus/Explicit, density) will be ignored; the userdefined material behavior requires that all mechanical material behavior calculations be programmed in subroutine UMAT or VUMAT. In Abaqus/Explicit the density (“Density,” Section 21.2.1) is required when using a user-defined material behavior.
| Input File Usage: | In Abaqus/Standard use the following option to specify a user-defined material behavior:*USER MATERIAL, TYPE=MECHANICAL,CONSTANTS=number_of_constantsIn Abaqus/Explicit use both of the following options to specify a user-defined material behavior:*USER MATERIAL, CONSTANTS=number_of_constants*DENSITYIn either case you must specify the number of material constants being entered. |
| Abaqus/CAE Usage: | In Abaqus/Standard use the following option to specify a user-defined material behavior:Property module: material editor: General→User Material:User material type: MechanicalIn Abaqus/Explicit use both of the following options to specify a user-defined material behavior:Property module: material editor:General→User Material: User material type: MechanicalGeneral→Density |
Unsymmetric equation solver in Abaqus/Standard
If the user material’s Jacobian matrix, , is not symmetric, the unsymmetric equation solution capability in Abaqus/Standard should be invoked (see “Defining an analysis,” Section 6.1.2).
Input File Usage:
*USER MATERIAL, TYPE=MECHANICAL,
CONSTANTS=number_of_constants, UNSYMM
Abaqus/CAE Usage:
Property module: material editor: General→User Material: User material type: Mechanical, toggle on Use unsymmetric material stiffness matrix
Hybrid formulation in Abaqus/Standard
If you use a hybrid element with user subroutine UMAT, by default Abaqus/Standard replaces the pressure stress calculated from the stress tensor returned by the user subroutine with that derived from the Lagrange multiplier and modifies the Jacobian appropriately (“Hybrid incompressible solid element formulation,” Section 3.2.3 of the Abaqus Theory Guide). This approach is suitable for material models that use an incremental formulation (for example, metal plasticity) but is not consistent with the total formulation that is commonly used for hyperelastic materials. In the latter situation the default formulation may lead to convergence problems. Such convergence problems may be observed, for example, when an almost incompressible nonlinear elastic user material is subjected to large deformations. Abaqus/Standard provides an alternate total formulation that is more appropriate in such situations. The total formulation is consistent with the native almost incompressible formulation used by Abaqus for hyperelastic materials (“Hyperelastic material behavior,” Section 4.6.1 of the Abaqus Theory Guide), and works better than the default (incremental) formulation for such cases.
Abaqus/Standard also provides a fully incompressible formulation for use with hybrid elements to define a fully incompressible user material response. The fully incompressible formulation is consistent with the native formulation used by Abaqus for incompressible hyperelastic materials. For the total hybrid formulation it is assumed that the deviatoric and the volumetric responses of the material are decoupled and that the volumetric response can be derived from a strain energy potential function. All the native hyperelastic materials in Abaqus use this assumption. For the incompressible hybrid formulation, it is assumed that the deviatoric stress can be derived from a strain energy potential function.
The total hybrid formulation is useful for an almost incompressible hyperelastic response. The volumetric response of the material is assumed to be defined in terms of an alternate variable, , in place of the volume change, . The alternate variable is made available inside user subroutine UMAT. Further details are discussed in “UMAT,” Section 1.1.44 of the Abaqus User Subroutines Reference Guide.
The fully incompressible formulation requires you to define only the deviatoric parts of the stress tensor and the material’s Jacobian matrix inside the UMAT. Abaqus/Standard automatically accounts for the pressure stress based on the Lagrange multiplier.
Input File Usage:
Use the following option to invoke the total hybrid formulation:
*USER MATERIAL, TYPE=MECHANICAL,
CONSTANTS=number_of_constants, HYBRID FORMULATION=TOTAL
Use following option to invoke the incremental hybrid formulation (default):
*USER MATERIAL, TYPE=MECHANICAL,
CONSTANTS=number_of_constants,
HYBRID FORMULATION=INCREMENTAL