Thermal Expansion

Abaqus requires thermal expansion coefficients, $\alpha$ , that define the total thermal expansion from a reference temperature, ${\theta }^0$ , as shown in Figure 1.

Figure 1. Definition of the thermal expansion coefficient.

They generate thermal strains according to the formula

where

$\alpha \left(\theta ,f_{\beta }\right)$

is the thermal expansion coefficient;

$\theta$

is the current temperature;

${\theta }^I$

is the initial temperature;

$f_{\beta }$

are the current values of the predefined field variables;

$f_{\beta }^I$

are the initial values of the field variables; and

${\theta }^0$

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, ${\theta }^I$ , and the reference temperature, ${\theta }^0$ . 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.

EXPANSION, ZERO=${\theta }^0$

Property module: material editor: MechanicalExpansion: Reference temperature: ${\theta }^0$

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 1). To convert to the total thermal expansion form required by Abaqus, this relationship must be integrated from a suitably chosen reference temperature, ${\theta }^0$ :

For example, suppose ${\alpha }^{\prime }$ is a series of constant values: ${\alpha }_1^{\prime }$ between ${\theta }^0$ and ${\theta }^1$ ; ${\alpha }_2^{\prime }$ between ${\theta }^1$ and ${\theta }^2$ ; ${\alpha }_3^{\prime }$ between ${\theta }^2$ and ${\theta }^3$ ; etc. Then,

The corresponding total expansion coefficients required by Abaqus are then obtained as

If an element has been removed and subsequently reactivated in Abaqus/Standard (Element and Contact Pair Removal and Reactivation), ${\theta }^I$ and $f_{\beta }^I$ in the equation for the thermal strains represent temperature and field variable values as they were at the moment of reactivation.

If the thermal expansion coefficient is defined directly, only one value of $\alpha$ is needed at each temperature. If user subroutine UEXPAN is used, only one isotropic thermal strain increment ( $\mathrm{\Delta }\epsilon =\mathrm{\Delta }{\epsilon }_{11}=\mathrm{\Delta }{\epsilon }_{22}=\mathrm{\Delta }{\epsilon }_{33}$ ) must be defined.

EXPANSION, TYPE=ISO

EXPANSION, TYPE=ISO, USER

Property module: material editor: MechanicalExpansion: Type: Isotropic

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

If the thermal expansion coefficients are defined directly, the three expansion coefficients in the principal material directions ( ${\alpha }_{11}$ , ${\alpha }_{22}$ , and ${\alpha }_{33}$ ) 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 ( $\mathrm{\Delta }{\epsilon }_{11}$ , $\mathrm{\Delta }{\epsilon }_{22}$ , and $\mathrm{\Delta }{\epsilon }_{33}$ ) must be defined.

EXPANSION, TYPE=ORTHO

EXPANSION, TYPE=ORTHO, USER

Property module: material editor: MechanicalExpansion: Type: Orthotropic

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

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, ${\alpha }_{22}={\alpha }_{33}$ . Only two expansion coefficients in the principal material directions ( ${\alpha }_{11}$ and ${\alpha }_{22}$ ) are needed as functions of temperature.

EXPANSION, TYPE=TRANSVERSELY ISOTROPIC

If the thermal expansion coefficients are defined directly, all six components of $\alpha$ ( ${\alpha }_{11}$ , ${\alpha }_{22}$ , ${\alpha }_{33}$ , ${\alpha }_{12}$ , ${\alpha }_{13}$ , ${\alpha }_{23}$ ) must be given as functions of temperature. If user subroutine UEXPAN is used in Abaqus/Standard, all six components of the thermal strain increment ( $\mathrm{\Delta }{\epsilon }_{11}$ , $\mathrm{\Delta }{\epsilon }_{22}$ , $\mathrm{\Delta }{\epsilon }_{33}$ , $\mathrm{\Delta }{\epsilon }_{12}$ , $\mathrm{\Delta }{\epsilon }_{13}$ , $\mathrm{\Delta }{\epsilon }_{23}$ ) must be defined. If user subroutine VUEXPAN is used in Abaqus/Explicit, all six components of the thermal strain increment ( $\mathrm{\Delta }{\epsilon }_{11}$ , $\mathrm{\Delta }{\epsilon }_{22}$ , $\mathrm{\Delta }{\epsilon }_{33}$ , $\mathrm{\Delta }{\epsilon }_{12}$ , $\mathrm{\Delta }{\epsilon }_{23}$ , $\mathrm{\Delta }{\epsilon }_{13}$ ) 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.

EXPANSION, TYPE=ANISO

EXPANSION, TYPE=ANISO, USER

Property module: material editor: MechanicalExpansion: Type: Anisotropic

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

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.