Spurious oscillations due to small time increments In transient heat transfer analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is $$ \Delta t > \frac {\rho c}{6 k} \Delta \ell^ {2}, $$ where is the time increment, is the density, c is the specific heat, k is the thermal conductivity, and $\Delta \ell$ is a typical element dimension (such as the length of a side of an element). If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly. There is no upper limit on the time increment size (the integration procedure is unconditionally stable) unless nonlinearities cause convergence problems. # Ending a transient analysis By default, a transient analysis will end when the specified time period has been completed. Alternatively, you can specify that the analysis should continue until steady-state conditions are reached. Steady state is defined by the temperature change rate; when the temperature changes at a rate that is less than the user-specified rate (given as part of the step definition), the analysis terminates.
Input File Usage:Use the following option to end the analysis when the time period is reached:*COUPLED THERMAL-ELECTRICAL, END=PERIOD (default)Use the following option to end the analysis based on the temperature change rate:*COUPLED THERMAL-ELECTRICAL, END=SS
Abaqus/CAE Usage:Step module: Create Step: General: Coupled thermal-electric: Basic: Response: Transient; Incrementation: End step when temperature change is less than
# Fully coupled solution schemes Abaqus/Standard offers an exact as well as an approximate implementation of Newton’s method for coupled thermal-electrical 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: $$ \left[ \begin{array}{c c} \boldsymbol {K} _ {\varphi \varphi} & \boldsymbol {K} _ {\varphi \theta} \\ \boldsymbol {K} _ {\theta \varphi} & \boldsymbol {K} _ {\theta \theta} \end{array} \right] \left\{ \begin{array}{c} \Delta \varphi \\ \Delta \boldsymbol {\theta} \end{array} \right\} = \left\{ \begin{array}{c} \boldsymbol {R} _ {\varphi} \\ \boldsymbol {R} _ {\theta} \end{array} \right\}, $$ where $\Delta \varphi$ and $\Delta \theta$ are the respective corrections to the incremental electrical potential and temperature, $K _ { i j }$ are submatrices of the fully coupled Jacobian matrix, and $R _ { \varphi }$ and $R _ { \theta }$ are the electrical and thermal residual vectors, respectively. Solving this system of equations requires the use of the unsymmetric matrix storage and solution scheme. Furthermore, the electrical 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 electrical and thermal solutions evolve simultaneously, but with a weak coupling between the two solutions. In other words, the components in the off-diagonal submatrices $K _ { \varphi \theta } , K _ { \theta \varphi }$ are small compared to the components in the diagonal submatrices $K _ { \varphi \varphi } , K _ { \theta \theta }$ . 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: $$ \left[ \begin{array}{c c} \boldsymbol {K} _ {\varphi \varphi} & 0 \\ 0 & \boldsymbol {K} _ {\theta \theta} \end{array} \right] \left\{ \begin{array}{c} \Delta \varphi \\ \Delta \theta \end{array} \right\} = \left\{ \begin{array}{c} \boldsymbol {R} _ {\varphi} \\ \boldsymbol {R} _ {\theta} \end{array} \right\}. $$ As a result of this approximation the electrical and thermal equations can be solved separately, with fewer equations to consider in each subproblem. The savings due to this approximation, measured as solver time per iteration, will be of the order of a factor of two, with similar significant savings in solver storage of the factored stiffness matrix. Further, in situations without strong thermal loading due to cavity radiation, the subproblems may be fully symmetric or approximated as symmetric, so that the less costly symmetric storage and solution scheme can be used. The solver time savings for a symmetric solution is an additional factor of two. Unless you explicitly select the unsymmetric solver for the step (“Defining an analysis,” Section 6.1.2), the symmetric solver will be used with this separated technique. This modified form of Newton’s method does not affect solution accuracy since the fully coupled effect is considered through the residual vector $R _ { j }$ at each increment in time. However, the rate of convergence is no longer quadratic and depends strongly on the magnitude of the coupling effect, so more iterations are generally needed to achieve equilibrium than with the exact implementation of Newton’s method. When the coupling is significant, the convergence rate becomes very slow and may prohibit the attainment of a solution. In such cases the exact implementation of Newton’s method is required. In cases where it is possible to use this approximation, the convergence in an increment will depend strongly on the quality of the first guess to the incremental solution, which you can control by selecting the extrapolation method used for the step (see “Defining an analysis,” Section 6.1.2). Input File Usage: Use the following option to specify a separated solution scheme: \*SOLUTION TECHNIQUE, TYPE=SEPARATED Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electric: Other: Solution technique: Separated # Uncoupled electric conduction and heat transfer analysis The coupled thermal-electrical procedure can also be used to perform uncoupled electric conduction analysis for the whole model or just part of the model (using coupled thermal-electrical elements). Uncoupled electrical analysis is available by omitting the thermal properties from the material description, in which case only the electric potential degrees of freedom are activated in the element and all heat transfer effects are ignored. If heat transfer effects are ignored in the entire model, you should invoke the separated solution technique described above. Use of this technique will then invoke the symmetric storage and solution scheme, which is an exact representation of a purely electrical problem. Similarly, coupled thermal-electrical elements can be used in an uncoupled heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2), in which case all electric conduction effects are ignored. This feature is useful if a thermal-electrical analysis is followed by a pure heat conduction analysis. A typical example is a welding process, where the electric current is applied instantaneously, followed by a cooldown period during which no electrical effects need to be considered. The symmetric solver is activated by default in an uncoupled heat transfer analysis. # Cavity radiation Cavity radiation can be activated in a heat transfer step. This feature involves interacting heat transfer between all of the facets of the cavity surface, dependent on the facet temperatures, facet emissivities, and the geometric view factors between each facet pair. When the thermal emissivity is a function of temperature or field variables, you can specify the maximum allowable emissivity change during an increment in addition to the maximum temperature change to control the time incrementation. See “Cavity radiation,” Section 41.1.1, for more information.
Input File Usage:Use the following option in the step definition to activate cavity radiation:*RADIATION VIEW FACTORUse the following option to specify the maximum allowable emissivity change:*HEAT TRANSFER, MXDEM=max_delta_emissivity
Abaqus/CAE Usage:You can specify the maximum allowable emissivity change for a heat transfer step.Step module:Create Step: General: Heat transfer: Incrementation:Max. allowable emissivity change per increment
# Initial conditions By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures or field variables (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Since only steady-state electrical currents are considered, the initial value of the electrical potential is not relevant. # Boundary conditions Boundary conditions can be used to prescribe the electrical potential, $\varphi = \varphi ( \mathbf { x } , t )$ (degree of freedom 9), and the temperature, $\theta = \theta ( \mathbf { x } , t )$ (degree of freedom 11), at the nodes. See “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1. Boundary conditions can be specified as functions of time by referring to amplitude curves (see “Amplitude curves,” Section 34.1.2). A boundary without any prescribed boundary conditions corresponds to an insulated surface. # Loads Both thermal and electrical loads can be applied in a coupled thermal-electrical analysis. # Applying thermal loads The following types of thermal loads can be prescribed in a coupled thermal-electrical analysis, as described in “Thermal loads,” Section 34.4.4: • Concentrated heat fluxes. • Body fluxes and distributed surface fluxes. • Average-temperature radiation conditions. • Convective film conditions and radiation conditions. # Applying electrical loads The following types of electrical loads can be prescribed, as described in “Electromagnetic loads,” Section 34.4.5: • Concentrated current. • Distributed surface current densities and body current densities. # Predefined fields Predefined temperature fields are not allowed in coupled thermal-electrical analyses. Boundary conditions should be used instead to specify temperatures, as described above. Other predefined field variables can be specified in a coupled thermal-electrical analysis. These values affect only field-variable-dependent material properties, if any. See “Predefined fields,” Section 34.6.1. # Material options Both thermal and electrical properties are active in coupled thermal-electrical analyses. If thermal properties are omitted, an uncoupled electrical analysis will be performed. All mechanical behavior material models (such as elasticity and plasticity) are ignored in a coupled thermal-electrical analysis. # Thermal material properties For the heat transfer portion of the analysis, the thermal conductivity must be defined (see “Conductivity,” Section 26.2.2). The specific heat must also be defined for transient heat transfer problems (see “Specific heat,” Section 26.2.3). If changes in internal energy due to phase changes are important, latent heat can be defined (see “Latent heat,” Section 26.2.4). Thermal expansion coefficients (“Thermal expansion,” Section 26.1.2) are not meaningful in a coupled thermal-electrical analysis since deformation of the structure is not considered. Internal heat generation can be specified (see “Uncoupled heat transfer analysis,” Section 6.5.2). # Electrical material properties For the electrical portion of the analysis, the electrical conductivity must be defined (see “Electrical conductivity,” Section 26.5.1). The electrical conductivity can be a function of temperature and user-defined field variables. The fraction of electrical energy dissipated as heat can also be defined, as explained above. # Elements The simultaneous solution in a coupled thermal-electrical analysis requires the use of elements that have both temperature (degree of freedom 11) and electrical potential (degree of freedom 9) as nodal variables. The finite element model can also include pure heat transfer elements (so that a pure heat transfer analysis is provided for that part of the model) and coupled thermal-electrical elements for which no thermal properties are given (so that a pure electrical conduction solution is provided for that part of the model). Coupled thermal-electrical elements are available in Abaqus/Standard in one dimension, two dimensions (planar and axisymmetric), and three dimensions. See “Choosing the appropriate element for an analysis type,” Section 27.1.3. # Output The following output variables can be used to request output relating to the electric conduction solution: Element integration point variables:
EPGMagnitude and components of the electrical potential gradient vector, $\partial \varphi / \partial \mathbf{x}$ .
EPGMMagnitude of the electrical potential gradient vector.
EPGnComponent $n$ of the electrical potential gradient vector ( $n=1, 2, 3$ ).
ECDMagnitude and components of the electrical current density vector, $J$ .
JENERElectrical energy dissipated due to flow of current, $P_{ec} t_{step}$ .
Whole element variables:
ECURSDistributed applied electrical current.
NCURSElectrical current at nodes due to electric conduction.
ELJDTotal electrical energy dissipated due to flow of current, $\int_{v} P_{ec} t_{step} dv$ .
Nodal variables:
EPOTElectrical potential, $\varphi$ .
RECURReactive electrical current.
CECURConcentrated applied electrical current.
Whole model variables: ALLJD Electrical energy summed over the model. Surface interaction variables (see “Electrical contact properties,” Section 37.3.1):
ECDElectrical current density.
ECDAECD multiplied by area.
ECDTTime integrated ECD.
ECDTATime integrated ECDA.
SJDHeat flux per unit area generated by the electrical current.
SJDASJD multiplied by area.
SJDTTime integrated SJD.
SJDTATime integrated SJDA.
WEIGHTHeat distribution between interface surfaces, f.
# Considerations for steady-state coupled thermal-electrical analysis In a steady-state coupled thermal-electrical analysis the electrical energy dissipated due to flow of electrical current at an integration point (output variable JENER) is computed using the following relationship: $$ E _ {e c} = P _ {e c} t _ {s t e p}, $$ where $E _ { e c }$ denotes the electrical energy dissipated due to flow of electrical current and $t _ { s t e p }$ is the current step time. In the above relationship it is assumed that the rate of the electrical energy dissipation, $P _ { e c ; }$ , has a constant value in the step that is equal to the value currently computed. The output variable JENER and the derived output variables ELJD and ALLJD contain the values of electrical energies dissipated in the current step only. Similarly, the contribution from the electrical current flow to the output variable ALLWK includes only the external work performed in the current step. # Input file template ```txt *HEADING ... *MATERIAL, NAME=mat1 *CONDUCTIVITY Data lines to define thermal conductivity ``` \*ELECTRICAL CONDUCTIVITY Data lines to define electrical conductivity \*JOULE HEAT FRACTION Data lines to define the fraction of electric energy released as heat \*\* \*STEP \*COUPLED THERMAL-ELECTRICAL Data line to define incrementation and steady state \*BOUNDARY Data lines to define boundary conditions on electrical potential and temperature degrees of freedom \*CECURRENT Data lines to define concentrated currents \*DECURRENT and/or \*DSECURRENT Data lines to define distributed current densities \*CFLUX and/or \*DFLUX and/or \*DSFLUX Data lines to define thermal loading \*FILM and/or \*SFILM and/or \*RADIATE and/or \*SRADIATE Data lines to define convective film and radiation conditions \*CONTACT PRINT or \*CONTACT FILE Data lines to request output of surface interaction variables \*END STEP # 6.7.4 FULLY COUPLED THERMAL-ELECTRICAL-STRUCTURAL ANALYSIS Products: Abaqus/Standard Abaqus/CAE # References • “Defining an analysis,” Section 6.1.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Coupled thermal-electrical analysis,” Section 6.7.3 • \*COUPLED TEMPERATURE-DISPLACEMENT • “Configuring a fully coupled, simultaneous heat transfer, electrical, and structural procedure” 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-electrical-structural analysis: • is performed when coupling between the displacement, temperature, and electrical potential fields makes it necessary to obtain solutions for all three fields simultaneously; • requires the existence of elements with displacement, temperature, and electrical potential degrees of freedom in the model; • allows for transient or steady-state thermal solutions, static displacement solutions, and steady-state electrical solutions; • can include thermal interactions such as gap radiation, gap conductance, and gap heat generation between surfaces (see “Thermal contact properties,” Section 37.2.1); • can include electrical interactions such as gap electrical conductance (see “Electrical contact properties,” Section 37.3.1); • cannot include cavity radiation effects but may include radiation boundary conditions (see “Thermal loads,” Section 34.4.4); • takes into account temperature dependence of material properties only for the properties that are assigned to elements with temperature degrees of freedom; • neglects inertia effects; and • can be transient or steady state. # Fully coupled thermal-electrical-structural analysis A fully coupled thermal-electrical-structural analysis is the union of a coupled thermal-displacement analysis (see “Fully coupled thermal-stress analysis,” Section 6.5.3) and a coupled thermal-electrical analysis (see “Coupled thermal-electrical analysis,” Section 6.7.3). Coupling between the temperature and electrical degrees of freedom arises from temperaturedependent electrical conductivity and internal heat generation (Joule heating), which is a function of the electrical current density. The thermal part of the problem can include heat conduction and heat storage (“Thermal properties: overview,” Section 26.2.1). Forced convection caused by fluid flowing through the mesh is not considered. Coupling between the temperature and displacement degrees of freedom arises from temperature-dependent material properties, thermal expansion, and internal heat generation, which is a function of inelastic deformation of the material. In addition, contact conditions exist in some problems where the heat conducted between surfaces may depend strongly on the separation of the surfaces and/or the pressure transmitted across the surfaces as well as friction (see “Mechanical contact properties: overview,” Section 37.1.1, and “Thermal contact properties,” Section 37.2.1). Coupling between the electrical and displacement degrees of freedom arises in problems where electricity flows between contact surfaces. The electrical conduction may depend strongly on the separation of the surfaces and/or the pressure transmitted across the surfaces (see “Electrical contact properties,” Section 37.3.1). An example of a simulation that requires a fully coupled thermal-electrical-structural analysis is resistance spot welding. In a typical spot welding process two or more thin metal sheets are pinched between two electrodes. A large current is passed between the electrodes, which melts the metal between the electrodes and forms a weld. The integrity of the weld depends on many parameters including the electrical conductance between the sheets (which can be a function of contact pressure and temperature). # Steady-state analysis Steady-state analysis provides the steady-state solution directly. Steady-state thermal analysis means that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. A static displacement solution is assumed. Only direct current is considered in the electrical problem, and it is assumed that the system has negligible capacitance. Electrical transient effects are so rapid that they can be neglected. Input File Usage: \*COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, STEADY STATE Abaqus/CAE Usage: Step module: Create Step: General: Coupled thermal-electricalstructural: Basic: Response: Steady state Assigning a “time” scale to the analysis In steady-state cases you should assign an arbitrary “time” scale to the step: you specify a “time” period and “time” incrementation parameters. This time scale is convenient for changing loads and boundary conditions through the step and for obtaining solutions to highly nonlinear (but steady-state) cases; however, for the latter purpose, transient analysis often provides a natural way of coping with the nonlinearity.