can be defined by specifying thermal expansion coefficients so that Abaqus can compute thermal strains;
can be isotropic, transversely isotropic, orthotropic, or fully anisotropic; or, for pore
fluids, can be isotropic only;
are defined as total expansion from a reference temperature;
can be defined as a tangent expansion in Abaqus/Standard;
can be specified as a function of temperature and/or field variables;
can be defined with a distribution for solid continuum elements in Abaqus/Standard;
can be specified directly in Abaqus/Standard in the user subroutine UEXPAN or in Abaqus/Explicit in user subroutine VUEXPAN if the thermal strains are
complicated functions of temperature, time, field variables, and state variables; and
can be defined independently for the solid grains and the pore fluid in a porous
medium.
Thermal 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
expansion must be used with the gasket behavior definition (see Defining the Gasket Behavior Directly Using a Gasket Behavior Model).
In an Abaqus/Standard analysis a spatially varying thermal expansion can be defined for homogeneous solid
continuum elements by using a distribution (Distribution Definition). The distribution
must include default values for the thermal expansion. If a distribution is used, no
dependencies on temperature and/or field variables for the thermal expansion can be defined.
Input File Usage
Use the following options to define thermal expansion for most materials:
Use the following option with other material behaviors, including gasket behavior, to
include thermal expansion effects:
Property module: material editor: MechanicalExpansion
Computation of Thermal Strains
In Abaqus, thermal expansion coefficients can define the total (or secant) thermal expansion or
the differential (or tangent) thermal expansion as shown in Figure 1.
Figure 1. Definition of the thermal expansion coefficient.
Secant Thermal Expansion
The secant thermal expansion coefficients, , define the thermal expansion from a reference temperature, , as shown in Figure 1.
They generate thermal strains according to the formula
where
is the secant thermal expansion coefficient;
is the current temperature;
is the initial temperature;
are the current values of the predefined field variables;
are the initial values of the field variables; and
is the reference temperature for the thermal expansion coefficient.
The second term in the above equation represents the strain arising from the difference
between the initial temperature, , and the reference temperature, . This term is necessary to enforce the assumption that there is no
initial thermal strain for cases in which the reference temperature does not equal the
initial temperature.
If the secant coefficient of thermal expansion, , is not a function of temperature or field variables, the value of the
reference temperature, , is not needed. If is a function of temperature or field variables, you can define .
Property module: material editor: MechanicalExpansion: Reference temperature:
Tangent Thermal Expansion in Abaqus/Standard
Abaqus/Standard also supports the definition of thermal expansion coefficients in tangent form. This
capability is particularly useful in situations when a material undergoes curing or
similar irreversible transformations and the thermal expansion coefficient depends on the
degree of transformation. Such processes are usually described using a differential (or
tangent) form of thermal expansion that cannot be generally expressed in total (or secant)
form because of the irreversible nature of the transformation.
The tangent coefficient of thermal expansion, , is the slope of the expansion curve at a given temperature (see Figure 1). If the tangent coefficient is
specified, the increment of the thermal strain is computed from
and the thermal strain, , is obtained by integrating the above equation from the initial to the
current temperature.
Because of the incremental nature of the formulation, the resulting thermal strains
generally depend on the temperature and field variable history and might be sensitive to
the time increment size (small time increments are preferred). Therefore, the general
recommendation is to use the total (secant) form except for the special situations of
irreversible processes where the tangent formulation can be more suitable to describe the
evolution of thermal strains.
You cannot specify tangent thermal expansion coefficients for short-fiber reinforced
composites, the pore fluid in the porous medium, and the
TNM model.
Defining tangent thermal expansion is not supported in Abaqus/CAE.
Converting Thermal Expansion Coefficients from Differential Form to Total Form
As discussed earlier, except for materials undergoing irreversible processes, the general
recommendation is to use the total form definition of thermal expansion because it leads
to thermal strain results that are not dependent on the temperature and field variable
history or sensitive to the time increment size. In addition, the total form is the only
option available in Abaqus/Explicit. Therefore, it is sometimes necessary to convert the thermal expansion coefficients
from the differential (tangent) to the total (secant) form. This conversion is always
possible when the thermal expansion coefficients are only a function of temperature (no
field variable dependency).
The temperature dependent tangent thermal expansion data has the form:
that is, the tangent to the strain-temperature curve is provided (see Figure 1). To convert to the secant thermal
expansion form required by Abaqus, this relationship must be integrated from a suitably chosen reference temperature, :
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
Computing Thermal Strains in Linear Perturbation Steps
During a linear perturbation step, temperature perturbations can produce perturbations of
thermal strains in the form:
where is the temperature perturbation load about the base state, is the temperature in the base state, and is the tangent thermal expansion coefficient evaluated in the base state.
If the secant thermal expansion coefficients are specified, Abaqus computes the tangent thermal expansion coefficients from the total form as
Defining Increments of Thermal Strain in User Subroutines
Increments of thermal strain can be specified in user subroutine UEXPAN in Abaqus/Standard and in user subroutine VUEXPAN in Abaqus/Explicit as functions of temperature and/or predefined field variables. User subroutine UEXPAN in Abaqus/Standard must be used if the thermal strain increments depend on state variables.
Property module: material editor: MechanicalExpansion: Use user subroutine UEXPAN
Defining the Initial Temperature and Field Variable Values
If the coefficient of thermal expansion, , is a function of temperature or field variables, the initial temperature
and initial field variable values, and , are given as described in Initial Conditions.
Element Removal and Reactivation
If an element has been removed and subsequently reactivated in Abaqus/Standard (Element and Contact Pair Removal and Reactivation), and in the equation for the thermal strains represent temperature and field
variable values as they were at the moment of reactivation.
Isotropic, orthotropic, and fully anisotropic thermal expansion can be defined in Abaqus.
Orthotropic and anisotropic thermal expansion can be used only with materials where the
material directions are defined with local orientations (see Orientations).
Isotropic Expansion
If the thermal expansion coefficient is defined directly, only one value of is needed at each temperature. If the user subroutine UEXPAN is used, only one isotropic
thermal strain increment () must be defined.
Input File Usage
Use the following option to define the thermal expansion coefficient
directly:
Use the following input to define the thermal expansion coefficient directly:
Property module: material editor: MechanicalExpansion: Type: Isotropic
Use the following input to define the thermal expansion with user subroutine UEXPAN:
Property module: material editor: MechanicalExpansion: Type: Isotropic, Use user subroutine UEXPAN
Orthotropic Expansion
If the thermal expansion coefficients are defined directly, the three expansion
coefficients in the principal material directions (, , and ) should be given as functions of temperature. If user subroutines UEXPAN and VUEXPAN are used, the three
components of thermal strain increment in the principal material directions (, , and ) must be defined.
Input File Usage
Use the following option to define the thermal expansion coefficient
directly:
Use the following input to define the thermal expansion coefficient directly:
Property module: material editor: MechanicalExpansion: Type: Orthotropic
Use the following input to define the thermal expansion with the user subroutine
UEXPAN:
Property module: material editor: MechanicalExpansion: Type: Orthotropic, Use user subroutine UEXPAN
Transversely Isotropic Expansion
A special subclass of orthotropy is transverse isotropy,
which is characterized by a plane of isotropy at every point in the material. Abaqus assumes the 2–3 plane to be the plane of isotropy at every point; therefore, . Only two expansion coefficients in the principal material directions ( and ) are needed as functions of temperature.
Input File Usage
Use the following option to define the thermal expansion coefficient
directly:
Defining thermal expansion for a transversely isotropic material is not supported in
Abaqus/CAE.
Anisotropic Expansion
If the thermal expansion coefficients are defined directly, all six components of (, , , , , ) must be given as functions of temperature. If user subroutine UEXPAN is used in Abaqus/Standard, all six components of the thermal strain increment (, , , , , ) must be defined. If user subroutine VUEXPAN is used in Abaqus/Explicit, all six components of the thermal strain increment (, , , , ,) must be defined.
In an Abaqus/Standard analysis if a distribution is used to define the thermal expansion, the number of
expansion coefficients given for each element in the distribution, which is determined by
the associated distribution table (Distribution Definition), must be
consistent with the level of anisotropy specified for the expansion behavior. For example,
if orthotropic behavior is specified, three expansion coefficients must be defined for
each element in the distribution.
Input File Usage
Use the following option to define the thermal expansion coefficient
directly:
Use the following input to define the thermal expansion coefficient directly:
Property module: material editor: MechanicalExpansion: Type: Anisotropic
Use the following input to define the thermal expansion with user subroutine UEXPAN:
Property module: material editor: MechanicalExpansion: Type: Anisotropic, Use user subroutine UEXPAN
Defining Thermal Expansion for a Short-Fiber Reinforced Composite
The thermal expansion coefficient of a short-fiber reinforced composite (for example, an
injection molded composite) can be computed using the orientation averaging described by
Zheng (2011):
where is the orientation-averaged elasticity matrix computed using the
elasticity of the unidirectional (UD) composite and the
second-order orientation tensor (see Defining the Elasticity of a Short-Fiber Reinforced Composite), and is given by:
where and are the elasticity matrix and thermal expansion coefficient of the
unidirectional composite with the 1-direction as the fiber direction, is the second-order orientation tensor, and is the Kronecker delta. The unidirectional composite is assumed to be
transversely isotropic. Similar to elasticity, you must define the material directions with
local orientations (see Orientations), and the axes of
the local system must align with the principal directions of the second-order orientation
tensor.
Input File Usage
Use the following option to define the transversely isotropic thermal expansion
coefficient of the unidirectional composite:
When a structure is not free to expand, a change in temperature will cause stress. For
example, consider a single two-node truss of length L that is
completely restrained at both ends. The cross-sectional area; the Young's modulus,
E; and the thermal expansion coefficient, , are all constant. The stress in this one-dimensional problem can then be
calculated from Hooke's Law as , where is the total strain and is the thermal strain, where is the temperature change. Since the element is fully restrained, . If the temperature at both nodes is the same, we obtain the stress .
Constrained thermal expansion can cause significant stress. For typical structural metals,
temperature changes of about 150°C (300°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.
Material Options
Thermal expansion can be combined with any other (mechanical) material (see Combining Material Behaviors) 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 by defining the incremental thermal strains in
user subroutine UEXPAN in Abaqus/Standard and VUEXPAN in Abaqus/Explicit. For porous media such as soils or rock, you can define thermal expansion for the solid
grains and for the permeating fluid (when using either the coupled pore fluid
diffusion/stress procedure in Abaqus/Standard or Abaqus/Explicit for the solid grains and for the permeating fluid using either the coupled pore fluid
diffusion/stress procedure—see Coupled Pore Fluid Diffusion and Stress Analysis—or undrained
pore fluid flow and stress analysis in Abaqus/Explicit—see Undrained Pore Fluid Flow and Stress Analysis ). In such
cases, you should repeat the thermal expansion definition to define the different thermal
expansion effects.
Using Thermal Expansion with Gasket Behaviors
Thermal expansion can be used 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.
Output
THE:
Thermal strain tensor (symmetric).
THEFL:
Thermal strain in the pore fluid in a porous medium (scalar).
References
Zheng, R., I. Tanner, and X. Fan, Injection Molding: Integration of Theory and Modeling
Methods, Springer, 2011.