ProductsAbaqus/Standard Defining field expansion coefficientsField expansion is a material property included in a material definition (see Material data definition) except when it refers to the expansion of a gasket whose material properties are not defined as part of a material definition. In that case field expansion must be used in conjunction with the gasket behavior definition (see Defining the gasket behavior directly using a gasket behavior model). Input File Usage Use the following options to define field expansion associated with predefined field variable number n for most materials: MATERIAL EXPANSION, FIELD=n The EXPANSION option can be repeated with different values of the predefined field variable number n to define field expansion associated with more than one field. Use the following options to define field expansion associated with predefined field variable number n for gaskets whose constitutive response is defined directly as gasket behavior: GASKET BEHAVIOR EXPANSION, FIELD=n The EXPANSION option can be repeated with different values of the predefined field variable number n to define field expansion associated with more than one field. Computation of field expansion strainsAbaqus/Standard requires field expansion coefficients, , that define the total field expansion from a reference value of the predefined field variable n, , as shown in Figure 1. Figure 1. Definition of the field expansion coefficient.
The field expansion for each specified field generates field expansion strains according to the formula where
The second term in the above equation represents the strain due to the difference between the initial value of the predefined field variablen, , and the corresponding reference value, . This term is necessary to enforce the assumption that there is no initial field expansion strain for cases in which the reference value of the predefined field variable n does not equal the corresponding initial value. Defining the reference value of the predefined field variableIf the coefficient of field expansion, , is not a function of temperature or field variables, the reference value of the predefined field variable, , is not needed. If is a function of temperature or field variables, you can define . Input File Usage EXPANSION, FIELD=n, ZERO= Converting field expansion coefficients from differential form to total formTotal field expansion coefficients can be provided directly as outlined in the previous section. However, you may have field expansion data available in differential form: that is, the tangent to the strain-field variable curve is provided (see Figure 1). To convert to the total field expansion form required by Abaqus, this relationship must be integrated from a suitably chosen reference value of the field variable, : For example, suppose is a series of constant values: between and ; between and ; between and ; etc. Then, The corresponding total expansion coefficients required by Abaqus are then obtained as Defining increments of field expansion strain in user subroutine UEXPANIncrements of field expansion strain can be specified in user subroutine UEXPAN as functions of temperature and/or predefined field variables. User subroutine UEXPAN must be used if the field expansion strain increments depend on state variables. You can use user subroutine UEXPAN only once within a single material definition. In particular, you cannot define both thermal and field expansions or multiple field expansions within the same material definition using user subroutine UEXPAN. Input File Usage EXPANSION, FIELD=n, USER Defining the initial temperature and field variable valuesIf the coefficient of field expansion, , is a function of temperature and/or predefined field variables, the initial temperature and initial predefined field variable values, and , are given as described in Initial conditions in Abaqus/Standard and Abaqus/Explicit. Element removal and reactivationIf an element has been removed and subsequently reactivated (Element and contact pair removal and reactivation), and in the equation for the field expansion strains represent temperature and predefined field variable values as they were at the moment of reactivation. Defining directionally dependent field expansionIsotropic, orthotropic, or fully anisotropic field expansion can be defined. Orthotropic and anisotropic field expansion can be used only with materials where the material directions are defined with local orientations (see Orientations). Only isotropic field expansion is allowed with the hyperelastic and hyperfoam material models. Isotropic expansionIf the field expansion coefficient is defined directly, only one value of is needed at each temperature and/or predefined field variable. If user subroutine UEXPAN is used, only one isotropic field expansion strain increment () must be defined. Orthotropic expansionIf the field expansion coefficients are defined directly, the three expansion coefficients in the principal material directions (, , and ) should be given as functions of temperature and/or predefined field variables. If user subroutine UEXPAN is used, the three components of field expansion strain increment in the principal material directions (, , and ) must be defined. Anisotropic expansionIf the field expansion coefficients are defined directly, all six components of (, , , , , ) must be given as functions of temperature and/or predefined field variables. If user subroutine UEXPAN is used, all six components of the field expansion strain increment (, , , , , ) must be defined. Field expansion stressWhen a structure is not free to expand, a change in a predefined field variable will cause stress if there is field expansion associated with that predefined field variable. For example, consider a single 2-node truss of length L that is completely restrained at both ends. The cross-sectional area; the Young's modulus, E; and the field expansion coefficient, , are all constants. The stress in this one-dimensional problem can then be calculated from Hooke's Law as , where is the total strain and is the field expansion strain, where is the change in the value of the predefined field variable number n. Since the element is fully restrained, . If the values of the field variable at both nodes are the same, we obtain the stress . Depending on the value of the field expansion coefficient and the change in the value of the corresponding predefined field variable, a constrained field expansion can cause significant stress and introduce strain energy that will result in an equivalent increase in the total energy of the model. Therefore, it is often important to define boundary conditions with particular care for problems involving this property to avoid overconstraining the field expansion. Material optionsField expansion can be combined with any other (mechanical) material (see Combining material behaviors) behavior in Abaqus/Standard. Using field expansion with other material modelsFor most materials field expansion is defined by a single coefficient or a set of orthotropic or anisotropic coefficients or by defining the incremental field expansion strains in user subroutine UEXPAN. Using field expansion with gasket behaviorField expansion can be used in conjunction with any gasket behavior definition. Field expansion will affect the expansion of the gasket in the membrane direction and/or the expansion in the gasket's thickness direction. ElementsField expansion can be used with any stress/displacement element in Abaqus/Standard, except for beam and shell elements using a general section behavior. |