Products: Abaqus/Standard Abaqus/CFD Abaqus/CAE
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.
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.
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, temperature-dependent 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.
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 temperature-dependent 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.
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 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 |
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.
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, 
, 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 |
| Abaqus/CAE Usage: | Step module: Create Step: General: Heat transfer: Response: Steady-state: Incrementation: Type: Fixed: Increment size: |
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
is the time increment, 
is the magnitude of the velocity vector, and 
is a characteristic element length in the direction of flow; that is, heat cannot be convected across more than one element length, , 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.
The time increments can be selected automatically based on the user-prescribed maximum allowable nodal temperature change in an increment, 
. 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: |
If you select direct incrementation and do not specify , fixed time increments equal to the user-specified initial time increment, , will then be used throughout the analysis.
| Input File Usage: | *HEAT TRANSFER |
| Abaqus/CAE Usage: | Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Fixed: Increment size: |
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
is the time increment, 
is the density, c is the specific heat, k is the thermal conductivity, and 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 
, where 
is the magnitude of the fluid velocity and is a characteristic element length in the direction of flow. Abaqus/Standard will adjust the time increment automatically to satisfy this stability limit.
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 |
Volumetric heat generation within a material can be defined either in user subroutine HETVAL or user subroutine UMATHT. These user subroutines are mutually exclusive.
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 |
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 |
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:
is the magnitude of the velocity vector, is the density, c is the specific heat, k is the thermal conductivity, and 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, . 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 occur, in particular if the flow is not precisely tangential to the boundary along which the temperature change occurs.
| Input File Usage: | Use the following option within the heat transfer step definition to prescribe the fluid velocity: |
*MASS FLOW RATE |
| Abaqus/CAE Usage: | Mass flow rate is not supported in Abaqus/CAE. |
By default, the mass flow rates given are modifications of existing flow rates or are to be applied in addition to any mass flow rates defined previously. You can remove all previously defined mass flow rates and, optionally, specify new mass flow rates.
| Input File Usage: | Use the following option to modify an existing flow rate or to specify an additional flow rate: |
*MASS FLOW RATE, OP=MOD (default) Use the following option to release all previously applied flow rates and to specify new flow rates: *MASS FLOW RATE, OP=NEW |
| Abaqus/CAE Usage: | Mass flow rate is not supported in Abaqus/CAE. |
Mass flow rates can be given in combination with an amplitude definition, if required, to control the magnitude of the flow rate as a function of time (“Amplitude curves,” Section 34.1.2).
| Input File Usage: | Use both of the following options to define a time-dependent mass flow rate: |
*AMPLITUDE, NAME=name *MASS FLOW RATE, AMPLITUDE=name |
| Abaqus/CAE Usage: | Mass flow rate is not supported in Abaqus/CAE. |
Mass flow rates can be defined by user subroutine UMASFL. UMASFL will be called for each specified node. Any mass flow rate values given directly will be ignored.
| Input File Usage: | *MASS FLOW RATE, USER |
| Abaqus/CAE Usage: | Mass flow rate is not supported in Abaqus/CAE. |
The data for the mass flow rate can be contained in an alternate file. See “Input syntax rules,” Section 1.2.1, for the syntax of the file name.
| Input File Usage: | *MASS FLOW RATE, INPUT=file_name |
| Abaqus/CAE Usage: | Mass flow rate is not supported in Abaqus/CAE. |
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 FACTOR Use 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 |
Uncoupled heat transfer analysis can be used in Abaqus/CFD to model heat conduction in solids provided there are no fluids in the model. This capability is distinct from fluid analysis with heat transfer, which is covered in “Fluid dynamic analysis,” Section 6.6. Solids should be modeled using fluid element types with a solid section type (see “Fluid element library,” Section 28.2.2). General temperature-dependent conductivity, convection, and radiation boundary conditions are supported. Nonlinearity can be introduced through temperature-dependent material properties and radiation boundary conditions. The solid heat transfer analysis is implemented using a finite volume formulation.
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. In this case the time incrementation input data are ignored, and Abaqus/CFD automatically iterates until steady-state conditions are reached. For output purposes the time increment size is set to unity, and simulation “time” can be interpreted as iteration count. Any fluxes or boundary conditions used in a steady-state heat transfer step should use values that are constant over time.
| Input File Usage: | *HEAT TRANSFER, CENTERING=ELEMENT, TYPE=THERMAL FLOW, STEADY STATE |
Transient analysis is conducted using the trapezoidal rule and a fixed time increment size that you specify. Material response is linearized over each time increment. Iterations are performed automatically within each increment when radiation boundary conditions are present.
| Input File Usage: | *HEAT TRANSFER, CENTERING=ELEMENT, TYPE=THERMAL FLOW |
The solution methods for heat conduction equations in Abaqus/CFD rely on scalable parallel preconditioned Krylov solvers. A set of preselected default convergence criteria and iteration limits are prescribed for all linear equation solvers. The default solver settings should provide computationally efficient and robust solutions across a spectrum of heat transfer problems. However, Abaqus/CFD provides full access to diagnostic information, convergence criteria, and optional solvers.
| Input File Usage: | *ENERGY EQUATION SOLVER |
By default, the initial temperature of all nodes is zero. You can specify nonzero initial temperatures (see “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).
In an Abaqus/Standard heat transfer analysis involving forced convection through the mesh, you can define nonzero initial mass flow rates at the nodes of the forced convection/diffusion heat transfer elements in the model, as described in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1.
For element types DCC1D2 and DCC1D2D the mass flow rate is positive from the first to the second node of the element. For two- and three-dimensional elements the direction of the mass flow rate is defined by giving the components in the x-, y-, and z-directions.
| Input File Usage: | *INITIAL CONDITIONS, TYPE=MASS FLOW RATE |
| Abaqus/CAE Usage: | Mass flow rate is not supported in Abaqus/CAE. |
In Abaqus/Standard, boundary conditions can be used to prescribe temperatures (degree of freedom 11) at nodes in a heat transfer analysis (see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1). Shell elements have additional temperature degrees of freedom 12, 13, etc. through the thickness (see “Conventions,” Section 1.2.2). Boundary conditions can be specified as functions of time by referring to amplitude curves (see “Amplitude curves,” Section 34.1.2).
In the finite volume formulation in Abaqus/CFD, temperature is an element-based degree of freedom. You can use boundary conditions to prescribe surface temperatures, and Abaqus/CFD computes element values that satisfy the heat conduction equations. See “Boundary conditions in Abaqus/CFD,” Section 34.3.2.
For purely diffusive heat transfer elements a boundary without any prescribed boundary conditions (natural boundary condition) corresponds to an insulated surface. For forced convection/diffusion elements only the flux associated with conduction is zero; energy is free to convect across an unconstrained surface. This natural boundary condition correctly models areas where fluid is crossing a surface (as, for example, at the upstream and downstream boundaries of the mesh) and prevents spurious reflections of energy back into the mesh.
The following types of loading can be prescribed in a heat transfer analysis, as described in “Thermal loads,” Section 34.4.4:
Concentrated heat fluxes (Abaqus/Standard only).
Body fluxes and distributed surface fluxes.
Average-temperature radiation conditions.
Convective film conditions and radiation conditions; film properties can be made a function of temperature.
Predefined temperature fields are not allowed in heat transfer analyses. Boundary conditions should be used instead to specify temperatures, as described earlier.
Other predefined field variables can be specified in a heat transfer analysis. These values will affect field-variable-dependent material properties, if any. See “Predefined fields,” Section 34.6.1.
The thermal conductivity of the materials in a heat transfer analysis must be defined. The specific heat and density of the materials must also be defined for transient heat transfer problems. Latent heat can be defined for diffusive heat transfer elements in Abaqus/Standard if changes in internal energy due to phase changes are important. Latent heat cannot be defined directly for forced convection/diffusion elements. See “Thermal properties: overview,” Section 26.2.1, for details on defining thermal properties in Abaqus.
Alternatively, user subroutine UMATHT can be used in Abaqus/Standard to define the thermal constitutive behavior of the material, including internal heat generation. For example, if a material modeled can go through a complex phase change, the specific heat can be defined in user subroutine UMATHT in sufficient detail to capture the phase change.
Thermal expansion coefficients are not meaningful in an uncoupled heat transfer analysis problem since deformation of the structure is not considered.
The heat transfer element library in Abaqus/Standard includes diffusive heat transfer elements, which allow for heat storage (specific heat and latent heat effects) and heat conduction.
Forced convection/diffusion heat transfer elements are also available in Abaqus/Standard: in addition to heat storage and heat conduction these elements allow for forced convection caused by fluid flowing through the mesh. These elements cannot be used with latent heat—see “Solid (continuum) elements,” Section 28.1.1, for additional details. Forced convection/diffusion elements with dispersion control are available for problems where the temperature transient in the fluid must be calculated accurately. See “Choosing the appropriate element for an analysis type,” Section 27.1.3.
Multiple temperatures are available through the thickness of shell heat transfer elements in Abaqus/Standard. See “Choosing a shell element,” Section 29.6.2.
The first-order heat transfer elements in Abaqus/Standard (such as the 2-node link, 4-node quadrilateral, and 8-node brick) use a numerical integration rule with the integration stations located at the corners of the element for the heat capacitance terms and for the calculations of the distributed surface fluxes. First-order diffusive elements are preferred in cases involving latent heat effects since they use such a special integration technique to provide accurate solutions with large latent heats. The forced convection/diffusion elements cannot use this special integration technique and, therefore, are unsuitable for problems with latent heat effects. The second-order heat transfer elements use conventional Gaussian integration. Thus, the second-order elements are to be preferred for problems when the solution will be smooth (without latent heat effects), and usually give more accurate results for the same number of nodes in the mesh.
Thermal interactions between adjacent surfaces and thermal gap elements are also provided in Abaqus/Standard to model heat transfer across the boundary layer between a solid and a fluid or between two closely adjacent solids. See “Thermal contact properties,” Section 37.2.1.
In Abaqus/CFD fluid elements should be used with solid sections to build uncoupled solid heat transfer models (see “Fluid element library,” Section 28.2.2). Fluid materials are not allowed in these models. This capability is distinct from fluid analysis with heat transfer, where fluid elements are used with fluid sections (see “Fluid dynamic analysis,” Section 6.6).
Different types of heat transfer output are available depending on whether you are performing an Abaqus/Standard or an Abaqus/CFD analysis.
The following heat transfer output variables are available:
HFL | Magnitude and components of the heat flux vector. |
HFLn | Component n of the heat flux vector (n=1, 2, 3). |
HFLM | Magnitude of the heat flux vector. |
TEMP | Integration point temperatures. |
MFR | User-specified mass flow rates. |
MFRn | Component n of the mass flow rate (n=1, 2, 3). |
FLUXS | Current values of uniform distributed heat fluxes. |
NFLUX | Fluxes at the nodes caused by heat conduction (internal fluxes). |
FILM | Current values of film conditions. |
RAD | Current values of radiation conditions. |
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 the node in forced convection/diffusion elements but excluding external fluxes due to user-defined concentrated fluxes, distributed fluxes, film conditions, radiation conditions, and cavity radiation. Since RFLE is a scalar nodal output variable, care should be taken when summing it over on two surfaces with shared nodes. If node sets on both surfaces include the shared nodes, the output of RFLE on the common nodes will contribute to the sums of this output quantity on both surfaces. |
RFLEn | Total flux value n at a node (n=11, 12, …). |
The following heat transfer output variables are available:
TEMP | Current values temperature. |
TEMP | Current values temperature. |
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. |
*HEADING … *PHYSICAL CONSTANTS, ABSOLUTE ZERO=*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,
*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=