| NT | Nodal point temperatures. |
| NTn | Temperature degree of freedom n at a node (n=11, 12, ...). |
| RFL | Reaction flux values due to prescribed temperature. |
| RFLn | Reaction flux value n at a node (n=11, 12, ...). |
| CFL | Concentrated flux values. |
| CFLn | Concentrated flux value n at a node (n=11, 12, ...). |
| RFLE | Total flux at a node, including flux convected through convection/diffusion elements but excluding external flux concentrated fluxes, distributed fluxes, film conditions, radiation cavity radiation. Since RFLE is a scalar nodal output value taken when summing it over on two surfaces with shared n both surfaces include the shared nodes, the output of RFLE will contribute to the sums of this output quantity on both s |
| RFLEn | Total flux value n at a node (n=11, 12, ...). |
All of the output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1.
# Output in Abaqus/CFD
The following heat transfer output variables are available:
Element variables:
TEMP Current values temperature.
Nodal variables:
TEMP Current values temperature.
Surface variables:
AVGTEMP Area-averaged surface temperature.
HEATFLOW Integrated normal heat flux on a surface. Heat flow is positive when heat is added to the system. This output request does not include the convective heat flow.
HFL Heat flux vector on a surface. This output request does not include the convective heat flow.
HFLN Normal heat flux on a surface. This output request does not include the convective heat flow.
All of the output variables available in Abaqus/CFD are listed in “Abaqus/CFD output variable identifiers,” Section 4.2.3.
Input file template
*HEADING
...
*PHYSICAL CONSTANTS, ABSOLUTE ZERO= $\theta^{Z}$ *INITIAL CONDITIONS, TYPE=TEMPERATURE
Data lines to prescribe initial temperatures at the nodes
*AMPLITUDE, NAME=trefamp
Data lines to define amplitude curve to be used for radiation reference temperature, $\theta^{0}$ *FILM PROPERTY, NAME=film
Data lines to define the convection film coefficient, h, as a function of temperature
**
*STEP
Transient analysis including forced convection through the mesh
*HEAT TRANSFER, END=SS, DELTMX= $\Delta\theta_{max}$ Data line to define incrementation and steady state
**
*CFLUX and/or *DFLUX
Data lines to define concentrated and/or distributed fluxes
*FILM
Data lines referring to film property table film
*RADIATE, AMPLITUDE=trefamp
Data lines to define boundary radiation
**
*EL PRINT
TEMP, HFL
NFLUX, FILM, RAD
*NODE PRINT
NT11, RFL
*END STEP
# 6.5.3 FULLY COUPLED THERMAL-STRESS ANALYSIS
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
# References
• “Defining an analysis,” Section 6.1.2
• “Heat transfer analysis procedures: overview,” Section 6.5.1
• \*COUPLED TEMPERATURE-DISPLACEMENT
• \*DYNAMIC TEMPERATURE-DISPLACEMENT
• “Specifying an inelastic heat fraction,” Section 12.10.3 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Configuring a fully coupled, simultaneous heat transfer and stress procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Configuring a dynamic fully coupled thermal-stress procedure using explicit integration” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
# Overview
A fully coupled thermal-stress analysis:
• is performed when the mechanical and thermal solutions affect each other strongly and, therefore, must be obtained simultaneously;
• requires the existence of elements with both temperature and displacement degrees of freedom in the model;
• can be used to analyze time-dependent material response;
• cannot include cavity radiation effects but may include average-temperature radiation conditions (see “Thermal loads,” Section 34.4.4); and
• takes into account temperature dependence of material properties only for the properties that are assigned to elements with temperature degrees of freedom.
In Abaqus/Standard a fully coupled thermal-stress analysis:
• neglects inertia effects; and
• can be transient or steady-state.
In Abaqus/Explicit a fully coupled thermal-stress analysis:
• includes inertia effects; and
• models transient thermal response.
# Fully coupled thermal-stress analysis
Fully coupled thermal-stress analysis is needed when the stress analysis is dependent on the temperature distribution and the temperature distribution depends on the stress solution. For example, metalworking problems may include significant heating due to inelastic deformation of the material which, in turn, changes the material properties. In addition, contact conditions exist in some problems where the heat conducted between surfaces may depend strongly on the separation of the surfaces or the pressure transmitted across the surfaces (see “Thermal contact properties,” Section 37.2.1). For such cases the thermal and mechanical solutions must be obtained simultaneously rather than sequentially. Coupled temperature-displacement elements are provided for this purpose in both Abaqus/Standard and Abaqus/Explicit; however, each program uses different algorithms to solve coupled thermal-stress problems.
# Fully coupled thermal-stress analysis in Abaqus/Standard
In Abaqus/Standard the temperatures are integrated using a backward-difference scheme, and the nonlinear coupled system is solved using Newton’s method. Abaqus/Standard offers an exact as well as an approximate implementation of Newton’s method for fully coupled temperature-displacement analysis.
# Exact implementation
An exact implementation of Newton’s method involves a nonsymmetric Jacobian matrix as is illustrated in the following matrix representation of the coupled equations:
$$
\left[ \begin{array}{c c} \boldsymbol {K} _ {\boldsymbol {u} \boldsymbol {u}} & \boldsymbol {K} _ {\boldsymbol {u} \boldsymbol {\theta}} \\ \boldsymbol {K} _ {\boldsymbol {\theta} \boldsymbol {u}} & \boldsymbol {K} _ {\boldsymbol {\theta} \boldsymbol {\theta}} \end{array} \right] \left\{ \begin{array}{c} \Delta \boldsymbol {u} \\ \Delta \boldsymbol {\theta} \end{array} \right\} = \left\{ \begin{array}{c} \boldsymbol {R} _ {\boldsymbol {u}} \\ \boldsymbol {R} _ {\boldsymbol {\theta}} \end{array} \right\},
$$
where $\Delta u$ and $\Delta \theta$ are the respective corrections to the incremental displacement and temperature, $K _ { i j }$ are submatrices of the fully coupled Jacobian matrix, and $\scriptstyle { R _ { u } }$ and $R _ { \theta }$ are the mechanical and thermal residual vectors, respectively.
Solving this system of equations requires the use of the unsymmetric matrix storage and solution scheme. Furthermore, the mechanical and thermal equations must be solved simultaneously. The method provides quadratic convergence when the solution estimate is within the radius of convergence of the algorithm. The exact implementation is used by default.
# Approximate implementation
Some problems require a fully coupled analysis in the sense that the mechanical and thermal solutions evolve simultaneously, but with a weak coupling between the two solutions. In other words, the components in the off-diagonal submatrices $K _ { u \theta } , \ K _ { \theta u }$ are small compared to the components in the diagonal submatrices $K _ { u u } , \ K _ { \theta \theta }$ . An example of such a situation is the disc brake problem (“Thermal-stress analysis of a disc brake,” Section 5.1.1 of the Abaqus Example Problems Guide). For these problems a less costly solution may be obtained by setting the off-diagonal submatrices to zero so that we obtain an approximate set of equations: