김경종
20 KiB
is the total strain and \varepsilon _ { x } ^ { t h } = \alpha \Delta \theta is the thermal strain, where \Delta \theta is the temperature change. Since the element is fully restrained, \varepsilon _ { x } = 0 . If the temperature at both nodes is the same, we obtain the stress \sigma _ { x } = - E \alpha \Delta \theta .
Constrained thermal expansion can cause significant stress. For typical structural metals, temperature changes of about 1 5 0 ^ { \circ } \mathrm { C } ~ ( 3 0 0 ^ { \circ } \mathrm { F } ) can cause yield. Therefore, it is often important to define boundary conditions with particular care for problems involving thermal loading to avoid overconstraining the thermal expansion.
Energy balance considerations
Abaqus does not account for thermal expansion effects in the total energy balance equation, which can lead to an apparent imbalance of the total energy of the model. For example, in the example above of a two-node truss restrained at both ends, constrained thermal expansion introduces strain energy that will result in an equivalent increase in the total energy of the model.
Use with other material models
Thermal expansion can be combined with any other (mechanical) material (see “Combining material behaviors,” Section 21.1.3) behavior in Abaqus.
Using thermal expansion with other material models
For most materials thermal expansion is defined by a single coefficient or set of orthotropic or anisotropic coefficients or, in Abaqus/Standard, by defining the incremental thermal strains in user subroutine UEXPAN. For porous media in Abaqus/Standard, such as soils or rock, thermal expansion can be defined for the solid grains and for the permeating fluid (when using the coupled pore fluid diffusion/stress procedure—see “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1). In such a case the thermal expansion definition should be repeated to define the different thermal expansion effects.
Using thermal expansion with gasket behaviors
Thermal expansion can be used in conjunction with any gasket behavior definition. Thermal expansion will affect the expansion of the gasket in the membrane direction and/or the expansion in the gasket’s thickness direction.
Elements
Thermal expansion can be used with any stress/displacement or fluid element in Abaqus.
26.1.3 FIELD EXPANSION
Product: Abaqus/Standard
References
• “Material library: overview,” Section 21.1.1
• “UEXPAN,” Section 1.1.30 of the Abaqus User Subroutines Reference Guide
• *EXPANSION
Overview
Field expansion effects:
• can be defined by specifying field expansion coefficients so that Abaqus/Standard can compute field expansion strains that are driven by changes in predefined field variables;
• can be isotropic, orthotropic, or fully anisotropic;
• are defined as total expansion from a reference value of the predefined field variable;
• can be specified as a function of temperature and/or predefined field variables;
• can be specified directly in user subroutine UEXPAN (if the field expansion strains are complicated functions of field variables and state variables); and
• can be defined for more than one predefined field variable.
Defining field expansion coefficients
Field expansion is a material property included in a material definition (see “Material data definition,” Section 21.1.2) 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,” Section 32.6.6).
Input File Usage:
Use the following options to define field expansion associated with predefined field variable number n for most materials:
\begin{array}{l} * \text { MATERIAL } \\ * \text { EXPANSION, FIELD } = n \end{array}
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:
\begin{array}{l} * \text { GASKET BEHAVIOR } \\ * \text { EXPANSION, FIELD } = n \\ \end{array}
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 strains
Abaqus/Standard requires field expansion coefficients, \alpha _ { f } , that define the total field expansion from a reference value of the predefined field variable n , f _ { n } ^ { 0 } . , as shown in Figure 26.1.3–1.
line
| f_n | ε^f (α_f)₁ | ε^f (α_f)₂ | ε^f (α_f)₁' | ε^f (α_f)₂' | | --- | --- | --- | --- | --- | | f_n^0 | 0 | 0 | 0 | 0 | | f_n^1 | ~0.5 | ~0.75 | ~0.6 | ~0.85 | | f_n^2 | ~1.0 | ~1.25 | ~1.1 | ~1.35 | | f_n | ~1.5 | ~1.75 | ~1.6 | ~1.85 |Figure 26.1.3–1 Definition of the field expansion coefficient.
The field expansion for each specified field generates field expansion strains according to the formula
\varepsilon^ {f} = \alpha_ {f} (\theta , f _ {\beta}) (f _ {n} - f _ {n} ^ {0}) - \alpha_ {f} (\theta^ {I}, f _ {\beta} ^ {I}) (f _ {n} ^ {I} - f _ {n} ^ {0}),
where
\begin{array}{l} \alpha_ {f} (\theta , f _ {\beta}) \quad \text { is the field expansion coefficient; } \\ f _ {n} \quad \text { is the current value of the predefined field variable } n; \\ f _ {n} ^ {I} \quad \text { is the initial value of the predefined field variable } n; \\ f _ {\beta} \quad \text { are the current values of the predefined field variables; } \\ \end{array}
f _ { \beta } ^ { I } are the initial values of the predefined field variables; and
f _ { n } ^ { 0 } is the reference value of the predefined field variable n for the field expansion coefficient.
The second term in the above equation represents the strain due to the difference between the initial value of the predefined field variablen, f _ { n } ^ { I } , and the corresponding reference value, f _ { n } ^ { 0 } . 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 variable
If the coefficient of field expansion, \alpha _ { f } , is not a function of temperature or field variables, the reference value of the predefined field variable, f _ { n } ^ { 0 } , is not needed. If \alpha _ { f } is a function of temperature or field variables, you can define f _ { n } ^ { 0 } . .
Input File Usage: *EXPANSION, FIELD=n, ZERO=
Converting field expansion coefficients from differential form to total form
Total field expansion coefficients can be provided directly as outlined in the previous section. However, you may have field expansion data available in differential form:
d \varepsilon^ {f} = \alpha_ {f} ^ {\prime} (f _ {n}) d f _ {n};
that is, the tangent to the strain-field variable curve is provided (see Figure 26.1.3–1). 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, f _ { n } ^ { 0 } . :
\varepsilon^ {f} = \int_ {f _ {n} ^ {0}} ^ {f _ {n}} \alpha_ {f} ^ {\prime} d f _ {n} \Rightarrow \alpha_ {f} (f _ {n}) = \frac {1}{f _ {n} - f _ {n} ^ {0}} \int_ {f _ {n} ^ {0}} ^ {f _ {n}} \alpha_ {f} ^ {\prime} d f _ {n}.
For example, suppose \alpha _ { f } ^ { \prime } is a series of constant values: \big ( \alpha _ { f } ^ { \prime } \big ) _ { 1 } between f _ { n } ^ { 0 } and f _ { n } ^ { 1 } ; ( \alpha _ { f } ^ { \prime } ) _ { 2 } between f _ { n } ^ { 1 } and f _ { n } ^ { 2 . } , ( \alpha ^ { \prime } ) _ { 3 } between f _ { n } ^ { 2 } and f _ { n } ^ { 3 } ; ; etc. Then,
\varepsilon_ {1} ^ {f} = (\alpha_ {f} ^ {\prime}) _ {1} (f _ {n} ^ {1} - f _ {n} ^ {0}),
\varepsilon_ {2} ^ {f} = \varepsilon_ {1} ^ {f} + (\alpha_ {f} ^ {\prime}) _ {2} (f _ {n} ^ {2} - f _ {n} ^ {1}),
\varepsilon_ {3} ^ {f} = \varepsilon_ {2} ^ {f} + (\alpha_ {f} ^ {\prime}) _ {3} (f _ {n} ^ {3} - f _ {n} ^ {2}).
The corresponding total expansion coefficients required by Abaqus are then obtained as
(\alpha_ {f}) _ {1} = \varepsilon_ {1} ^ {f} / (f _ {n} ^ {1} - f _ {n} ^ {0}),
(\alpha_ {f}) _ {2} = \varepsilon_ {2} ^ {f} / (f _ {n} ^ {2} - f _ {n} ^ {0}),
(\alpha_ {f}) _ {3} = \varepsilon_ {3} ^ {f} / (f _ {n} ^ {3} - f _ {n} ^ {0}).
Defining increments of field expansion strain in user subroutine UEXPAN
Increments 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 values
If the coefficient of field expansion, \alpha _ { f } . , is a function of temperature and/or predefined field variables, the initial temperature and initial predefined field variable values, \theta ^ { I } and f _ { \beta } ^ { I } , are given as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.
Element removal and reactivation
If an element has been removed and subsequently reactivated (“Element and contact pair removal and reactivation,” Section 11.2.1), \theta ^ { I } and f _ { \beta } ^ { I } 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 expansion
Isotropic, 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,” Section 2.2.5).
Only isotropic field expansion is allowed with the hyperelastic and hyperfoam material models.
Isotropic expansion
If the field expansion coefficient is defined directly, only one value of \alpha _ { f } is needed at each temperature and/or predefined field variable. If user subroutine UEXPAN is used, only one isotropic field expansion strain increment ( \Delta \varepsilon ^ { f } = \Delta \varepsilon _ { 1 1 } ^ { f } = \Delta \varepsilon _ { 2 2 } ^ { f } = \Delta \varepsilon _ { 3 3 } ^ { f } ) must be defined.
Input File Usage: Use the following option to define the field expansion coefficient directly:
\ast \mathrm { E X P A N S I O N } , \mathrm { F I E L D } = n , \mathrm { T Y P E } = \mathrm { I S O }
Use the following option to define the field expansion with user subroutine UEXPAN:
\ast \mathrm { E X P A N S I O N } , \mathrm { F I E L D } = n , \mathrm { T Y P E } = \mathrm { I S O } , \mathrm { U S E R }
Orthotropic expansion
If the field expansion coefficients are defined directly, the three expansion coefficients in the principal material directions ( \alpha _ { f _ { 1 1 } } , \alpha _ { f _ { 2 2 } } , \mathrm { a n d } \alpha _ { f _ { 3 3 } } ) 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 ( \Delta \varepsilon _ { 1 1 } ^ { f } , \Delta \varepsilon _ { 2 2 } ^ { f } , and \Delta \varepsilon _ { 3 3 } ^ { f } ) must be defined.
Input File Usage:
Use the following option to define the field expansion coefficients directly:
*EXPANSION, FIELD=n, TYPE=ORTHO
Use the following option to define the field expansion with user subroutine UEXPAN:
*EXPANSION, FIELD=n, TYPE=ORTHO, USER
Anisotropic expansion
If the field expansion coefficients are defined directly, all six components of ( , , , \alpha _ { f } \ ( \alpha _ { f _ { 1 1 } } , \alpha _ { f _ { 2 2 } } , \alpha _ { f _ { 3 3 } } , \alpha _ { f _ { 1 2 } } , \alpha _ { f _ { 1 3 } } , \alpha _ { f _ { 2 3 } } ) 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 ( \Delta \varepsilon _ { 1 1 } ^ { f } , \Delta \varepsilon _ { 2 2 } ^ { f } , \Delta \varepsilon _ { 3 3 } ^ { f } , \Delta \varepsilon _ { 1 2 } ^ { f } , \Delta \varepsilon _ { 1 3 } ^ { f } , \Delta \varepsilon _ { 2 3 } ^ { f } ) must be defined.
Input File Usage:
Use the following option to define the field expansion coefficients directly:
*EXPANSION, FIELD=n, TYPE=ANISO
Use the following option to define the field expansion with user subroutine UEXPAN:
*EXPANSION, FIELD=n, TYPE=ANISO, USER
Field expansion stress
When 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 _ { \mathrm { { \scriptscriptstyle 3 } } } and the field expansion coefficient, \alpha _ { f } , are all constants. The stress in this one-dimensional problem can then be calculated from Hooke’s Law as \sigma _ { x } = E ( \varepsilon _ { x } - \varepsilon _ { x } ^ { f } ) , where \varepsilon _ { x } is the total strain and \varepsilon _ { x } ^ { f } = \alpha _ { f } \Delta f _ { n } is the field expansion strain, where \Delta f _ { n } is the change in the value of the predefined field variable number n. Since the element is fully restrained, \varepsilon _ { x } = 0 . If the values of the field variable at both nodes are the same, we obtain the stress \sigma _ { x } = - E \alpha _ { f } \Delta f _ { n } .
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.
Use with other material models
Field expansion can be combined with any other (mechanical) material (see “Combining material behaviors,” Section 21.1.3) behavior in Abaqus/Standard.
Using field expansion with other material models
For 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 behavior
Field 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.
Elements
Field expansion can be used with any stress/displacement element in Abaqus/Standard, except for beam and shell elements using a general section behavior.
26.1.4 VISCOSITY
Products: Abaqus/Explicit Abaqus/CFD Abaqus/CAE
References
• “Viscous shear behavior” in “Equation of state,” Section 25.2.1
• *VISCOSITY
• *EOS
• *TRS
• “Defining viscosity” in “Defining other mechanical models,” Section 12.9.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
Material shear viscosity is an internal property of a fluid that offers resistance to flow. It can be specified in Abaqus/Explicit and Abaqus/CFD.
Material shear viscosity in Abaqus/Explicit:
• can be a function of temperature and shear strain rate; and
• must be used in combination with an equation of state (“Equation of state,” Section 25.2.1).
Material shear viscosity in Abaqus/CFD:
• can be a function of temperature only for the Newtonian model;
• can be a function of shear strain rate; and
• is not supported for field-dependent variants.
Viscous shear behavior
The resistance to flow of a viscous fluid is described by the following relationship between deviatoric stress and strain rate
\mathbf {S} = 2 \eta \dot {\mathbf {e}} = \eta \dot {\boldsymbol {\gamma}},
where is the deviatoric stress, is the deviatoric part of the strain rate, is the viscosity, and { \dot { \gamma } } = 2 { \dot { \mathbf { e } } } is the engineering shear strain rate.
Newtonian fluids are characterized by a viscosity that only depends on temperature, \eta ( \theta ) . In the more general case of non-Newtonian fluids the viscosity is a function of the temperature and shear strain rate:
\eta = \eta (\dot {\gamma}, \theta),
where \dot { \gamma } = \sqrt { \frac { 1 } { 2 } \dot { \gamma } : \dot { \gamma } } is the equivalent shear strain rate. In terms of the equivalent shear stress, \tau = \sqrt { { \textstyle { \frac { 1 } { 2 } } } \mathbf { S } : \mathbf { S } } , we have:
\tau = \eta \dot {\gamma}.
Non-Newtonian fluids can be classified as shear-thinning (or pseudoplastic), when the apparent viscosity decreases with increasing shear rate, and shear-thickening (or dilatant), when the viscosity increases with strain rate.
In addition to the Newtonian viscous fluid model, Abaqus/CFD and Abaqus/Explicit support several models of nonlinear viscosity to describe non-Newtonian fluids: power law, Carreau-Yasuda, Cross, Herschel-Bulkley, Powell-Eyring, and Ellis-Meter. Other functional forms of the viscosity can also be specified in tabular format. In addition, in Abaqus/Explicit user subroutine VUVISCOSITY can be used.
Newtonian
The Newtonian model is useful to model viscous laminar flow governed by the Navier-Poisson law of a Newtonian fluid, \tau = \eta \dot { \gamma } . Newtonian fluids are characterized by a viscosity that depends only on temperature, \eta ( \theta ) . You need to specify the viscosity as a tabular function of temperature when you define the Newtonian viscous deviatoric behavior.
Input File Usage: *VISCOSITY, DEFINITION=NEWTONIAN (default)
Abaqus/CAE Usage: Property module: material editor: Mechanical→Viscosity
Power law
The power law model is commonly used to describe the viscosity of non-Newtonian fluids. The viscosity is expressed as
\eta = k \dot {\gamma} ^ {n - 1}; \quad \eta_ {\mathrm{min}} \leq \eta \leq \eta_ {\mathrm{max}},
where is the flow consistency index and is the flow behavior index. When n \ < \ 1 , the fluid is shear-thinning (or pseudoplastic): the apparent viscosity decreases with increasing shear rate. When n > 1 , the fluid is shear-thickening (or dilatant); and when n = 1 , the fluid is Newtonian. Optionally, you can place a lower limit, \eta _ { \mathrm { { m i n } ; } } and/or an upper limit, \eta _ { \mathrm { m a x } } . , on the value of the viscosity computed from the power law.
Input File Usage: *VISCOSITY, DEFINITION=POWER LAW
Abaqus/CAE Usage: The power law model is not supported in Abaqus/CAE.
Carreau-Yasuda
The Carreau-Yasuda model describes the shear thinning behavior of polymers. This model often provides a better fit than the power law model for both high and low shear strain rates. The viscosity is expressed as