ProductsAbaqus/StandardAbaqus/CAE ## Fully coupled thermal-electrical-structural analysisA fully coupled thermal-electrical-structural analysis is the union of a coupled thermal-displacement analysis (see Fully coupled thermal-stress analysis) and a coupled thermal-electrical analysis (see Coupled thermal-electrical analysis). Coupling between the temperature and electrical degrees of freedom arises from temperature-dependent 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 (About thermal properties). 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 About mechanical contact properties and Thermal contact properties). 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). 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 analysisSteady-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-electrical-structural: Basic: Response: Steady state ## Assigning a “time” scale to the analysisIn 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. ## Accounting for frictional slip heat generationFrictional slip heat generation is normally neglected in the steady-state case. However, it can still be accounted for if user subroutine FRIC provides the incremental frictional dissipation through the variable SFD. If frictional heat generation is present, the heat flux into the two contact surfaces depends on the slip rate of the surfaces. The “time” scale in this case cannot be described as arbitrary, and a transient analysis should be performed. ## Transient analysisAlternatively, you can perform a transient coupled thermal-electrical-structural analysis. As in steady-state analysis, electrical transient effects are neglected and a static displacement solution is assumed. You can control the time incrementation in a transient analysis directly, or Abaqus/Standard can control it automatically. Automatic time incrementation is generally preferred. ## Automatic incrementation controlled by a maximum allowable temperature changeThe time increments can be selected automatically based on a user-prescribed maximum allowable nodal temperature change in an increment, $\mathrm{\Delta}{\theta}_{max}$. Abaqus/Standard will restrict the time increments to ensure that this value is not exceeded at any node (except nodes with boundary conditions) during any increment of the analysis (see Time integration accuracy in transient problems). Input File Usage COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX=$\mathrm{\Delta}{\theta}_{max}$ Abaqus/CAE Usage Step module: Create Step: General: Coupled thermal-electrical-structural: Basic: Response: Transient; Incrementation: Type: Automatic: Max. allowable temperature change per increment: $\mathrm{\Delta}{\theta}_{max}$ ## Fixed incrementationIf you do not specify $\mathrm{\Delta}{\theta}_{max}$, fixed time increments equal to the user-specified initial time increment, $\mathrm{\Delta}{t}_{0}$, will be used throughout the analysis, except when the explicit creep integration scheme is used. In this case Abaqus/Standard might decrease the time increment if the stability limit is exceeded. Input File Usage COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL $\mathrm{\Delta}{t}_{0}$ Abaqus/CAE Usage Step module: Create Step: General: Coupled thermal-electrical-structural: Basic: Response: Transient; Incrementation: Type: Fixed: Increment size: $\mathrm{\Delta}{t}_{0}$ ## Spurious oscillations due to small time incrementsIn transient analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. A simple guideline is $$\mathrm{\Delta}t>\frac{\rho c}{6k}\mathrm{\Delta}{\mathrm{\ell}}^{2},$$
where $\mathrm{\Delta}t$ is the time increment, $\rho $ is the density, c is the specific heat, k is the thermal conductivity, and $\mathrm{\Delta}\mathrm{\ell}$ 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. ## Automatic incrementation controlled by the creep responseThe accuracy of the integration of time-dependent (creep) material behavior is governed by the user-specified accuracy tolerance parameter, $tolerance\ge \left(\dot{\overline{\epsilon}}^{cr}{}_{t+\mathrm{\Delta}t}-\dot{\overline{\epsilon}}^{cr}{}_{t}\right)\mathrm{\Delta}t$. This parameter is used to prescribe the maximum strain rate change allowed at any point during an increment, as described in Rate-dependent plasticity: creep and swelling. The accuracy tolerance parameter can be specified together with the maximum allowable nodal temperature change in an increment, $\mathrm{\Delta}{\theta}_{max}$ (described above); however, specifying the accuracy tolerance parameter activates automatic incrementation even if $\mathrm{\Delta}{\theta}_{max}$ is not specified. Input File Usage COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX=$\mathrm{\Delta}{\theta}_{max}$, CETOL=tolerance Abaqus/CAE Usage Step module: Create Step: General: Coupled thermal-electrical-structural: Basic: Response: Transient, toggle on Include creep/swelling/viscoelastic behavior; Incrementation: Type: Automatic: Max. allowable temperature change per increment: $\mathrm{\Delta}{\theta}_{max}$, Creep/swelling/viscoelastic strain error tolerance: tolerance ## Selecting explicit creep integrationNonlinear creep problems (Rate-dependent plasticity: creep and swelling) that exhibit no other nonlinearities can be solved efficiently by forward-difference integration of the inelastic strains if the inelastic strain increments are smaller than the elastic strains. This explicit method is efficient computationally because, unlike implicit methods, iteration is not required as long as no other nonlinearities are present. Although this method is only conditionally stable, the numerical stability limit of the explicit operator is in many cases sufficiently large to allow the solution to be developed in a reasonable number of time increments. For most coupled thermal-electrical-structural analyses, however, the unconditional stability of the backward difference operator (implicit method) is desirable. In such cases the implicit integration scheme may be invoked automatically by Abaqus/Standard. Explicit integration can be less expensive computationally and simplifies implementation of user-defined creep laws in user subroutine CREEP; you can restrict Abaqus/Standard to using this method for creep problems (with or without geometric nonlinearity included). See Rate-dependent plasticity: creep and swelling for further details. Input File Usage COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, CETOL=tolerance, CREEP=EXPLICIT Abaqus/CAE Usage Step module: Create Step: General: Coupled thermal-electrical-structural: Basic: Response: Transient, toggle on Include creep/swelling/viscoelastic behavior; Incrementation: Creep/swelling/viscoelastic strain error tolerance: tolerance, Creep/swelling/viscoelastic integration: Explicit ## Excluding creep and viscoelastic responseYou can specify that no creep or viscoelastic response will occur during a step even if creep or viscoelastic material properties have been defined. Input File Usage COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL, DELTMX=$\mathrm{\Delta}{\theta}_{max}$, CREEP=NONE Abaqus/CAE Usage Step module: Create Step: General: Coupled thermal-electrical-structural: Basic: Response: Transient, toggle off Include creep/swelling/viscoelastic behavior ## Unstable problemsSome types of analyses may develop local instabilities, such as surface wrinkling, material instability, or local buckling. In such cases it may not be possible to obtain a quasi-static solution, even with the aid of automatic incrementation. Abaqus/Standard offers a method of stabilizing this class of problems by applying damping throughout the model in such a way that the viscous forces introduced are sufficiently large to prevent instantaneous buckling or collapse but small enough not to affect the behavior significantly while the problem is stable. The available automatic stabilization schemes are described in detail in Automatic stabilization of unstable problems. ## UnitsIn coupled problems where two or three different fields are active, take care when choosing the units of the problem. If the choice of units is such that the terms generated by the equations for each field are different by many orders of magnitude, the precision on some computers may be insufficient to resolve the numerical ill-conditioning of the coupled equations. Therefore, choose units that avoid ill-conditioned matrices. For example, consider using units of Mpascal instead of pascal for the stress equilibrium equations to reduce the disparity between the magnitudes of the stress equilibrium equations, the heat flux continuity equations, and the conservation of charge equations. ## Initial conditionsBy default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures. Initial stresses, field variables, etc. can also be defined; Initial conditions in Abaqus/Standard and Abaqus/Explicit describes all of the initial conditions that are available for a fully coupled thermal-electrical-structural analysis. ## Boundary conditionsBoundary conditions can be used to prescribe temperatures (degree of freedom 11), displacements/rotations (degrees of freedom 1–6), or electrical potentials (degree of freedom 9) at nodes in a fully coupled thermal-electrical-structural analysis (see Boundary conditions in Abaqus/Standard and Abaqus/Explicit). Boundary conditions can be specified as functions of time by referring to amplitude curves (Amplitude Curves). ## LoadsThe following types of thermal loads can be prescribed in a fully coupled thermal-electrical-structural analysis, as described in Thermal loads: -
Concentrated heat fluxes. -
Body fluxes and distributed surface fluxes. -
Node-based film and radiation conditions. -
Average-temperature radiation conditions. -
Element and surface-based film and radiation conditions.
The following types of mechanical loads can be prescribed: -
Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6); see Concentrated loads. -
Distributed pressure forces or body forces can be applied; see Distributed loads.
The following types of electrical loads can be prescribed, as described in Electromagnetic loads: -
Concentrated current. -
Distributed surface current densities and body current densities.
## Predefined fieldsPredefined temperature fields are not allowed in a fully coupled thermal-electrical-structural analysis. Boundary conditions should be used instead to prescribe temperature degree of freedom 11, as described earlier. Other predefined field variables can be specified in a fully coupled thermal-electrical-structural analysis. These values will affect only field-variable-dependent material properties, if any. See Predefined Fields. ## Material optionsThe materials in a fully coupled thermal-electrical-structural analysis must have thermal properties (such as conductivity), mechanical properties (such as elasticity), and electrical properties (such as electrical conductivity) defined. See Abaqus Materials Guide for details on the material models available in Abaqus. Internal heat generation can be specified; see Uncoupled heat transfer analysis. Thermal strain will arise if thermal expansion (Thermal expansion) is included in the material property definition. A fully coupled thermal-electrical-structural analysis can be used to analyze static creep and swelling problems, which generally occur over fairly long time periods (Rate-dependent plasticity: creep and swelling); viscoelastic materials (Time domain viscoelasticity); or viscoplastic materials (Rate-dependent yield). ## Inelastic energy dissipation as a heat sourceYou can specify an inelastic heat fraction in a fully coupled thermal-electrical-structural analysis to provide for inelastic energy dissipation as a heat source. The heat flux per unit volume, ${r}^{pl}$, that is added into the thermal energy balance is computed using the equation $${r}^{pl}=\eta \mathit{\sigma}:{\dot{\mathit{\epsilon}}}^{pl},$$
or, in the case when the nonlinear isotropic/kinematic hardening model is used, from the following equation: $${r}^{pl}=\eta \left(\mathit{\sigma}-\mathit{\alpha}\right):{\dot{\mathit{\epsilon}}}^{pl},$$
where $\eta $ is a user-defined factor (assumed constant), $\mathit{\sigma}$ is the stress, $\mathit{\alpha}$ is the backstress, and ${\dot{\mathit{\epsilon}}}^{pl}$ is the rate of plastic straining. Inelastic heat fractions are typically used in the simulation of high-speed manufacturing processes involving large amounts of inelastic strain, where the heating of the material caused by its deformation significantly influences temperature-dependent material properties. The generated heat is treated as a volumetric heat flux source term in the heat balance equation. An inelastic heat fraction can be specified for materials with plastic behavior that use the Mises or Hill yield surface (Inelastic behavior). It cannot be used with the combined isotropic/kinematic hardening model. The inelastic heat fraction can be specified for user-defined material behavior in Abaqus/Explicit and will be multiplied by the inelastic energy dissipation coded in the user subroutine to obtain the heat flux. In Abaqus/Standard the inelastic heat fraction cannot be used with user-defined material behavior; in this case the heat flux that must be added to the thermal energy balance is computed directly in the user subroutine. In Abaqus/Standard an inelastic heat fraction can also be specified for hyperelastic material definitions that include time-domain viscoelasticity (Time domain viscoelasticity). The default value of the inelastic heat fraction is 0.9. If you do not include the inelastic heat fraction behavior in the material definition, the heat generated by inelastic deformation is not included in the analysis. Input File Usage INELASTIC HEAT FRACTION $\eta $ Abaqus/CAE Usage Property module: material editor: Thermal: Inelastic Heat Fraction: Fraction: $\eta $ ## Specifying the amount of thermal energy generated due to electrical currentJoule's law describes the rate of electrical energy, ${P}_{ec}$, dissipated by current flowing through a conductor as $${P}_{ec}=\mathbf{J}\cdot \mathbf{E}=\frac{\partial \phi}{\partial \mathbf{x}}\cdot {\mathit{\sigma}}^{E}\cdot \frac{\partial \phi}{\partial \mathbf{x}}.$$
The amount of this energy released as internal heat within the body is ${\eta}_{v}{P}_{ec}$, where ${\eta}_{v}$ is an energy conversion factor. You specify ${\eta}_{v}$ in the material definition. It is assumed that all the electrical energy is converted into heat (${\eta}_{v}=1.0$) if you do not include the joule heat fraction in the material description. The fraction given can include a unit conversion factor, if required. Input File Usage JOULE HEAT FRACTION Abaqus/CAE Usage `Property module: material editor: ThermalJoule Heat Fraction` ## ElementsCoupled thermal-electrical-structural elements that have displacements, temperatures, and electrical potentials as nodal variables are available. Simultaneous temperature/electrical potential/displacement solution requires the use of such elements; pure displacement and temperature-displacement elements can be used in part of the model in a fully coupled thermal-electrical-structural analysis, but pure heat transfer elements cannot be used. The first-order coupled thermal-electrical-structural elements in Abaqus use a constant temperature over the element to calculate thermal expansion. The second-order coupled thermal-electrical-structural elements in Abaqus use a lower-order interpolation for temperature than for displacement (parabolic variation of displacements and linear variation of temperature) to obtain a compatible variation of thermal and mechanical strain. ## OutputSee Abaqus/Standard output variable identifiers for a complete list of output variables. The types of output available are described in About Output. ## Considerations for steady-state coupled thermal-electrical-structural analysisIn a steady-state coupled thermal-electrical-structural analysis the electrical energy dissipated due to flow of electrical current at an integration point (output variable JENER) is computed using the following relationship: $${E}_{ec}={P}_{ec}{t}_{step},$$
where ${E}_{ec}$ denotes the electrical energy dissipated due to flow of electrical current and ${t}_{step}$ is the current step time. In the above relationship it is assumed that the rate of the electrical energy dissipation, ${P}_{ec}$, 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 templateHEADING … ** Specify the coupled thermal-electrical-structural element type ELEMENT, TYPE=Q3D8 … ** STEP COUPLED TEMPERATURE-DISPLACEMENT, ELECTRICAL Data line to define incrementation BOUNDARY Data lines to define nonzero boundary conditions on displacement, temperature or electrical potential degrees of freedom CFLUX and/or CFILM and/or CRADIATE and/or DFLUX and/or DSFLUX and/or FILM and/or SFILM and/or RADIATE and/or SRADIATE Data lines to define thermal loads CLOAD and/or DLOAD and/or DSLOAD Data lines to define mechanical loads CECURRENT Data lines to define concentrated currents DECURRENT and/or DSECURRENT Data lines to define distributed current densities FIELD Data lines to define field variable values END STEP |