20.1.2 Thermal expansion

Products: ABAQUS/Standard  ABAQUS/Explicit  ABAQUS/CAE  

References

Overview

Thermal expansion effects:

  • can be defined by specifying thermal expansion coefficients so that ABAQUS can compute thermal strains;

  • can be isotropic, orthotropic, or fully anisotropic;

  • are defined as total expansion from a reference temperature;

  • can be specified as a function of temperature and/or field variables; and

  • in ABAQUS/Standard can be specified directly in user subroutine UEXPAN (if the thermal strains are complicated functions of field variables and state variables).

Defining thermal expansion coefficients

Thermal expansion is a material property included in a material definition (see Material data definition, Section 16.1.2) 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 expansion must be used in conjunction with the gasket behavior definition (see Defining the gasket behavior directly using a gasket behavior model, Section 26.6.6).

Input File Usage:           Use the following options to define thermal expansion for most materials:
*MATERIAL
*EXPANSION

Use the following options to define thermal expansion for gaskets whose constitutive response is defined directly as gasket behavior:

*GASKET BEHAVIOR
*EXPANSION

ABAQUS/CAE Usage: Use the following option in conjunction with other material behaviors, including gasket behavior, to include thermal expansion effects:

Property module: material editor: MechanicalExpansion


Computation of thermal strains

ABAQUS requires thermal expansion coefficients, , that define the total thermal expansion from a reference temperature, , as shown in Figure 20.1.2–1.

Figure 20.1.2–1 Definition of the thermal expansion coefficient.

They generate thermal strains according to the formula

where

is the 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 due to 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.

Defining the reference temperature

If the 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 .

Input File Usage:           
*EXPANSION, ZERO=

ABAQUS/CAE Usage: 

Property module: material editor: MechanicalExpansion: Reference temperature:


Converting thermal expansion coefficients from differential form to total form

Total thermal expansion coefficients are commonly available in tables of material properties. However, sometimes you are given thermal expansion data in differential form:

that is, the tangent to the strain-temperature curve is provided (see Figure 20.1.2–1). To convert to the total 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

Defining increments of thermal strain in user subroutine UEXPAN

Increments of thermal strain can be specified in ABAQUS/Standard user subroutine UEXPAN as functions of temperature and/or predefined field variables. User subroutine UEXPAN must be used if the thermal strain increments depend on state variables.

Input File Usage:           
*EXPANSION, USER

ABAQUS/CAE Usage: 

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, Section 27.2.1.

Element removal and reactivation

If an element has been removed and subsequently reactivated in ABAQUS/Standard (Element and contact pair removal and reactivation, Section 11.2.1), and in the equation for the thermal strains represent temperature and field variable values as they were at the moment of reactivation.

Defining directionally dependent thermal expansion

Isotropic or orthotropic thermal expansion can be defined in ABAQUS. In addition, fully anisotropic thermal expansion can be defined in ABAQUS/Standard.

Orthotropic and anisotropic thermal expansion can be used only with materials where the material directions are defined with local orientations (see Orientations, Section 2.2.5).

Orthotropic thermal expansion in ABAQUS/Explicit is allowed only with anisotropic elasticity (including orthotropic elasticity) and anisotropic yield (see Anisotropic yield/creep, Section 18.2.6).

Only isotropic thermal expansion is allowed for adiabatic stress analysis and with the hyperelastic and hyperfoam material models.

Isotropic expansion

If the thermal expansion coefficient is defined directly, only one value of is needed at each temperature.

Input File Usage:           
*EXPANSION, TYPE=ISO

ABAQUS/CAE Usage: 

Property module: material editor: MechanicalExpansion: Type: Isotropic


If user subroutine UEXPAN is used, only one isotropic thermal strain increment () must be defined.

Input File Usage:           
*EXPANSION, TYPE=ISO, USER

ABAQUS/CAE Usage: 

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.

Input File Usage:           
*EXPANSION, TYPE=ORTHO

ABAQUS/CAE Usage: 

Property module: material editor: MechanicalExpansion: Type: Orthotropic


If user subroutine UEXPAN is used, the three components of thermal strain increment in the principal material directions (, , and ) must be defined.

Input File Usage:           
*EXPANSION, TYPE=ORTHO, USER

ABAQUS/CAE Usage: 

Property module: material editor: MechanicalExpansion: Type: Orthotropic, Use user subroutine UEXPAN


Anisotropic expansion

If the thermal expansion coefficients are defined directly, all six components of (, , , , , ) must be given as functions of temperature.

Input File Usage:           
*EXPANSION, TYPE=ANISO

ABAQUS/CAE Usage: 

Property module: material editor: MechanicalExpansion: Type: Anisotropic


If user subroutine UEXPAN is used, all six components of the thermal strain increment (, , , , , ) must be defined.

Input File Usage:           
*EXPANSION, TYPE=ANISO, USER

ABAQUS/CAE Usage: 

Property module: material editor: MechanicalExpansion: Type: Anisotropic, Use user subroutine UEXPAN


Thermal stress

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 150C (300F) 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.

Use with other material properties or behaviors

Thermal expansion can be combined with any other (mechanical) material (see Combining material behaviors, Section 16.1.3) 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 6.7.1). 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 element in ABAQUS.