# 6.5 Heat transfer and thermal-stress analysis • “Heat transfer analysis procedures: overview,” Section 6.5.1 • “Uncoupled heat transfer analysis,” Section 6.5.2 • “Fully coupled thermal-stress analysis,” Section 6.5.3 • “Adiabatic analysis,” Section 6.5.4 # 6.5.1 HEAT TRANSFER ANALYSIS PROCEDURES: OVERVIEW Abaqus can solve the following types of heat transfer problems: • Uncoupled heat transfer analysis: Heat transfer problems involving conduction, forced convection, and boundary radiation can be analyzed in Abaqus/Standard or Abaqus/CFD. See “Uncoupled heat transfer analysis,” Section 6.5.2. In these analyses the temperature field is calculated without knowledge of the stress/deformation state or the electrical field in the bodies being studied. Pure heat transfer problems can be transient or steady-state and linear or nonlinear. • Sequentially coupled thermal-stress analysis: If the stress/displacement solution is dependent on a temperature field but there is no inverse dependency, a sequentially coupled thermal-stress analysis can be conducted in Abaqus/Standard. Sequentially coupled thermal-stress analysis is performed by first solving the pure heat transfer problem, then reading the temperature solution into a stress analysis as a predefined field. See “Sequentially coupled thermal-stress analysis,” Section 16.1.2. In the stress analysis the temperature can vary with time and position but is not changed by the stress analysis solution. Abaqus allows for dissimilar meshes between the heat transfer analysis model and the thermal-stress analysis model. Temperature values will be interpolated based on element interpolators evaluated at nodes of the thermal-stress model. • Fully coupled thermal-stress analysis: A coupled temperature-displacement procedure is used to solve simultaneously for the stress/displacement and the temperature fields. A coupled analysis is used when the thermal and mechanical solutions affect each other strongly. For example, in rapid metalworking problems the inelastic deformation of the material causes heating, and in contact problems the heat conducted across gaps may depend strongly on the gap clearance or pressure. Both Abaqus/Standard and Abaqus/Explicit provide coupled temperature-displacement analysis procedures, but the algorithms used by each program differ considerably. In Abaqus/Standard the heat transfer equations are integrated using a backward-difference scheme, and the coupled system is solved using Newton’s method. These problems can be transient or steady-state and linear or nonlinear. In Abaqus/Explicit the heat transfer equations are integrated using an explicit forward-difference time integration rule, and the mechanical solution response is obtained using an explicit central-difference integration rule. Fully coupled thermal-stress analysis in Abaqus/Explicit is always transient. Cavity radiation effects cannot be included in a fully coupled thermal-stress analysis. See “Fully coupled thermal-stress analysis,” Section 6.5.3, for more details. • Fully coupled thermal-electrical-structural analysis: A coupled thermal-electrical-structural procedure is used to solve simultaneously for the stress/displacement, the electrical potential, and the temperature fields. A coupled analysis is used when the thermal, electrical, and mechanical solutions affect each other strongly. An example of such a process is resistance spot welding, where two or more metal parts are joined by fusion at discrete points at the material interface. The fusion is caused by heat generated due to the current flow at the contact points, which depends on the pressure applied at these points. These problems can be transient or steady-state and linear or nonlinear. Cavity radiation effects cannot be included in a fully coupled thermal-electrical-structural analysis. This procedure is available only in Abaqus/Standard. See “Fully coupled thermal-electrical-structural analysis,” Section 6.7.4, for more details. • Adiabatic analysis: An adiabatic mechanical analysis can be used in cases where mechanical deformation causes heating, but the event is so rapid that this heat has no time to diffuse through the material. Adiabatic analysis can be performed in Abaqus/Standard or Abaqus/Explicit; see “Adiabatic analysis,” Section 6.5.4. An adiabatic analysis can be static or dynamic and linear or nonlinear. • Coupled thermal-electrical analysis: A fully coupled thermal-electrical analysis capability is provided in Abaqus/Standard for problems where heat is generated due to the flow of electrical current through a conductor. See “Coupled thermal-electrical analysis,” Section 6.7.3. • Cavity radiation: In Abaqus/Standard cavity radiation effects can be included (in addition to prescribed boundary radiation) in uncoupled heat transfer problems. See “Cavity radiation,” Section 41.1.1. The cavities can be open or closed. Symmetries and blocking within cavities can be modeled. view factors are calculated automatically, and motion of objects bounding a cavity can be prescribed during the analysis. Cavity radiation problems are nonlinear and can be transient or steady-state. # 6.5.2 UNCOUPLED HEAT TRANSFER ANALYSIS Products: Abaqus/Standard Abaqus/CFD Abaqus/CAE # References • “Defining an analysis,” Section 6.1.2 • “Heat transfer analysis procedures: overview,” Section 6.5.1 • \*HEAT TRANSFER • “Including volumetric heat generation in heat transfer analyses,” Section 12.10.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide • “Configuring a heat transfer 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 Uncoupled heat transfer problems: • are those in which the temperature field is calculated without consideration of the stress/deformation or the electrical field in the bodies being studied; • can include conduction, boundary convection, and boundary radiation; • can be transient or steady-state; and • can be linear or nonlinear. In Abaqus/Standard uncoupled heat transfer problems: • involve heat transfer in solid bodies; • can include cavity radiation effects—see “Cavity radiation,” Section 41.1.1; • can include forced convection through the mesh if forced convection/diffusion heat transfer elements are used; • can include thermal interactions such as gap radiation, conductance, and heat generation between contact surfaces—see “Thermal contact properties,” Section 37.2.1; • can include thermal material behavior defined in user subroutine UMATHT—see “User-defined thermal material behavior,” Section 26.7.2; and • require the use of heat transfer elements. In Abaqus/CFD uncoupled heat transfer problems: • involve heat transfer in solid bodies; • must not involve fluid flow; and • require the use of a fluid element type with a solid section—see “Fluid element library,” Section 28.2.2. Uncoupled heat transfer analysis is used to model solid body heat conduction with general, temperaturedependent conductivity, internal energy (including latent heat effects), and quite general convection and radiation boundary conditions, including cavity radiation. Forced convection of a fluid through the mesh can be modeled by using forced convection/diffusion elements. # Sources of nonlinearity in a heat transfer analysis Heat transfer problems can be nonlinear because the material properties are temperature dependent or because the boundary conditions are nonlinear. Usually the nonlinearity associated with temperaturedependent material properties is mild because the properties do not change rapidly with temperature. However, when latent heat effects are included, the analysis may be severely nonlinear (see “Latent heat,” Section 26.2.4). Boundary conditions are very often nonlinear; for example, film coefficients can be functions of surface temperature. Again, the nonlinearities are often mild and cause little difficulty. An exception is the “boiling” film condition, in which the film coefficient can change very rapidly because the fluid adjacent to the surface boils. A rapidly changing film condition (within a step or from one step to another) can be modeled easily using temperature-dependent and field-variable-dependent film coefficients. Radiation effects always make heat transfer problems nonlinear. Nonlinearities in radiation grow as temperatures increase. Abaqus/Standard uses an iterative scheme to solve nonlinear heat transfer problems. The scheme uses the Newton method with some modifications to improve stability of the iteration process in the presence of highly nonlinear latent heat effects. Steady-state cases involving severe nonlinearities are sometimes more effectively solved as transient cases because of the stabilizing influence of the heat capacity terms. The required steady-state solution can be obtained as the very long transient time response; the transient will simply stabilize the solution for that long time response. # Matrix storage and solution scheme In heat transfer analyses involving cavity radiation or forced convection/diffusion elements, the system of equations is unsymmetric. The nonsymmetric matrix storage and solution scheme is invoked automatically in these cases (see “Defining an analysis,” Section 6.1.2). # Steady-state analysis Steady-state analysis means that the internal energy term (the specific heat term) in the governing heat transfer equation is omitted. The problem then has no intrinsic physically meaningful time scale. Nevertheless, you can assign an initial time increment, a total time period, and maximum and minimum allowed time increments to the analysis step, which is often convenient for output identification and for specifying prescribed temperatures and fluxes with varying magnitudes. Any fluxes or boundary condition changes to be applied during a steady-state heat transfer step should be given within the step, using appropriate amplitude references to specify their “time” variations (“Amplitude curves,” Section 34.1.2). If fluxes and boundary conditions are specified for the step without amplitude references, they are assumed to change linearly with “time” during the step, from their magnitudes at the end of the previous step (or zero, if this is the beginning of the analysis) to their newly specified magnitudes at the end of the heat transfer step. Input File Usage: \*HEAT TRANSFER, STEADY STATE Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Steady state # Automatic incrementation When steady-state analysis is chosen, you suggest an initial “time” increment and define a “time” period for the step; Abaqus/Standard then increments through the step accordingly. By default, Abaqus/Standard automatically determines a suitable increment size for each increment of the step. # Fixed incrementation You can also use a fixed incrementation scheme, in which Abaqus/Standard uses the same increment size for the duration of the step. The suggested initial “time” increment, $\Delta t _ { 0 }$ , defines the increment size. Input File Usage: Set the initial increment, minimum increment size, and maximum increment size to the same value: \*HEAT TRANSFER, STEADY STATE $$ \Delta t _ {0},, \Delta t _ {0}, \Delta t _ {0} $$ Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Steady-state: Incrementation: Type: Fixed: Increment size: $\Delta t _ { 0 }$ # Transient analysis Time integration in transient problems is done with the backward Euler method (sometimes also referred to as the modified Crank-Nicholson operator) in the pure conduction elements. This method is unconditionally stable for linear problems. The forced convection/diffusion elements use the trapezoidal rule for time integration. They include numerical diffusion control (the “upwinding” Petrov-Galerkin method) and, optionally, numerical dispersion control. The elements with dispersion control offer improved solution accuracy in cases where the transient response of the fluid is important. Artificial dispersion control introduces a stability limit on the size of the time increment such that the local Courant number $$ C = | \mathbf {v} | \frac {\Delta t}{\Delta \ell} $$ must be less than 1, where $\Delta t$ is the time increment, is the magnitude of the velocity vector, and $\Delta \ell$ is a characteristic element length in the direction of flow; that is, heat cannot be convected across more than one element length, $\Delta \ell ,$ in a single increment of time. In a uniform velocity field the smallest element will dictate the stable time increment. Approximate calculation of the Courant number, C, is helpful during the mesh design stages so that excessively small stable time increments can be avoided. The elements without dispersion control have no such stability limit; therefore, it may be more economical to use the elements without this feature in transient cases where transient effects in the fluid itself are not a critical part of the solution (for example, when the important solution is the temperature field in the solid bodies that are included in the model, and when characteristic transient times in the fluid are very much shorter than characteristic transient times in the solids). Time incrementation in a transient heat transfer analysis can be controlled directly by you or automatically by Abaqus/Standard. Automatic time incrementation is generally preferred. # Automatic incrementation The time increments can be selected automatically based on the user-prescribed maximum allowable nodal temperature change in an increment, $\Delta \theta _ { m a x }$ . 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,” Section 7.2.4). Input File Usage: \*HEAT TRANSFER, DELTMX= Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Automatic: Max. allowable temperature change per increment: $\Delta \theta _ { m a x }$ # Fixed incrementation If you select direct incrementation and do not specify $\Delta \theta _ { m a x }$ , fixed time increments equal to the userspecified initial time increment, $\Delta t _ { 0 }$ , will then be used throughout the analysis. Input File Usage: \*HEAT TRANSFER $\Delta t _ { 0 }$ Abaqus/CAE Usage: Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Fixed: Increment size: $\Delta t _ { 0 }$ # 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 $\Delta t$ is the time increment, $\rho$ 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. Abaqus/Standard provides no check on the user-defined initial time increment; you must ensure that the given value does not violate the above criterion. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions especially in terms of the heat flux for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes occur. Unless you specify a maximum allowable time increment size as part of the heat transfer step definition, there is no upper limit on the time increment size (the integration procedure is unconditionally stable, at least for linear problems). However, if forced convection/diffusion elements including numerical dispersion control (element types DCCxxD) are included in the model, there is a numerical stability limit on the allowable time increment. The requirement is that $\Delta t \leq \Delta \ell / | { \bf v } |$ , where is the magnitude of the fluid velocity and $\Delta \ell$ is a characteristic element length in the direction of flow. Abaqus/Standard will adjust the time increment automatically to satisfy this stability limit. # Ending a transient analysis A transient analysis can be terminated by completing a specified time period, or it can be continued until steady-state conditions are reached. By default, the analysis will end when the given time period has been completed. Alternatively, you can specify that the analysis will end when steady state is reached or after the given time period, whichever comes first. Steady state is defined by the temperature change rate: when the temperature at every temperature degree of freedom 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:*HEAT TRANSFER, END=PERIOD (default)Use the following option to end the analysis based on the temperature change rate:*HEAT TRANSFER, END=SS

Abaqus/CAE Usage:

Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: End step when temperature change is less than

# Internal heat generation Volumetric heat generation within a material can be defined either in user subroutine HETVAL or user subroutine UMATHT. These user subroutines are mutually exclusive. # Defining internal heat generation in user subroutine HETVAL If user subroutine HETVAL is used to define internal heat generation, heat generation must be included in the material definition with the other thermal property definitions. Heat generation might be associated with (relatively low) energy phase changes occurring during the solution. Such heat generation usually depends on state variables (such as the fraction transformed), which themselves evolve with the solution and are stored as solution-dependent state variables (see “User subroutines: overview,” Section 18.1.1). The heat generation is computed in user subroutine HETVAL, where any associated state variables can also be updated. The subroutine will be called at all material calculation points for which the material definition includes heat generation. Input File Usage: \*HEAT GENERATION Abaqus/CAE Usage: Property module: material editor: Thermal: Heat Generation Defining internal heat generation in user subroutine UMATHT If user subroutine UMATHT is used to define internal heat generation, all other thermal properties must also be defined within the subroutine. Input File Usage: \*USER MATERIAL Abaqus/CAE Usage: Property module: material editor: General: User Material: User material type: Thermal # Forced convection through the mesh The velocity of a fluid moving through the mesh can be prescribed if forced convection/diffusion heat transfer elements are used. Conduction between the fluid and adjacent forced convection/diffusion heat transfer elements will be affected by the mass flow rate of the fluid. For example, if a pipe is filled with a fluid with an initial temperature profile that contains a temperature pulse, the initial temperature pulse will not only diffuse (because of conduction in the fluid and the pipe), but it will also be transported (or convected) down the pipe. Since the fluid velocity is prescribed, it is called forced convection. Natural convection occurs when differences in fluid density created by thermal gradients cause motion of the fluid (bouyancy-driven flow). The forced convection/diffusion elements are not designed to handle this phenomenon; the flow must be prescribed. You can specify the mass flow rates per unit area (or through the entire section for one-dimensional elements) at the nodes. Abaqus/Standard interpolates the mass flow rates to the material points. The numerical solution of the transient heat transfer equation including convection becomes increasingly difficult as convection dominates diffusion. The Peclet number, , is a dimensionless parameter that indicates the degree of convection dominance over diffusion: $$ \gamma = | \mathbf {v} | \Delta \ell \frac {\rho c}{k}, $$ where $| \mathbf { v } |$ is the magnitude of the velocity vector, is the density, c is the specific heat, k is the thermal conductivity, and $\Delta \ell$ is a characteristic element length in the direction of flow. Large values of indicate that convection dominates over diffusion on the spatial scale defined by the element size, $\Delta \ell .$ In general, Peclet numbers greater than about 1000 should not be used. Petrov-Galerkin finite elements are used in Abaqus/Standard to model systems with high Peclet numbers accurately; these elements use nonsymmetric, upwinded weighting functions to control numerical diffusion and dispersion and, thus, stabilize results. The upwinding term is partly a function of the element Peclet number, as described in “Convection/diffusion,” Section 2.11.3 of the Abaqus Theory Guide. If the fluid flows along a boundary along which a rapid change of temperature is prescribed, it is, in fact, subjected to a thermal transient, even for steady-state analysis. This transient can give rise to the same kind of spurious temperature oscillations that are observed in transient heat transfer analysis, as discussed earlier in this section. Since Abaqus/Standard uses first-order elements for convective heat transfer, the oscillation can be eliminated by lumping the heat capacity terms. However, the upwinded weighting functions prevent lumping in the direction of the flow. Hence, spurious oscillations may still