Uncoupled 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 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).

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).

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). 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.

HEAT TRANSFER, STEADY STATE

Step module: Create Step: General: Heat transfer: Response:
Steady state

HEAT TRANSFER, STEADY STATE
$\mathrm{\Delta }{t}_0$, , $\mathrm{\Delta }{t}_0$, $\mathrm{\Delta }{t}_0$

Step module: Create Step: General: Heat transfer: Response: Steady-state: Incrementation: Type: Fixed: Increment size: $\mathrm{\Delta }{t}_0$

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

must be less than 1, where $\mathrm{\Delta }t$ is the time increment, $\left|\mathbf{v}\right|$ is the magnitude of the velocity vector, and $\mathrm{\Delta }\mathrm{\ell }$ is a characteristic element length in the direction of flow; that is, heat cannot be convected across more than one element length, $\mathrm{\Delta }\mathrm{\ell }$, 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.

HEAT TRANSFER, DELTMX=$\mathrm{\Delta }{\theta }_{max}$

Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Automatic: Max. allowable temperature change per increment: $\mathrm{\Delta }{\theta }_{max}$

HEAT TRANSFER
$\mathrm{\Delta }{t}_0$

Step module: Create Step: General: Heat transfer: Response: Transient: Incrementation: Type: Fixed: Increment size: $\mathrm{\Delta }{t}_0$

HEAT TRANSFER, END=PERIOD (default)

HEAT TRANSFER, END=SS

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.

HEAT GENERATION

Property module: material editor: Thermal: Heat Generation

USER MATERIAL

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, $\gamma$, is a dimensionless parameter that indicates the degree of convection dominance over diffusion:

where $\left|\mathbf{v}\right|$ is the magnitude of the velocity vector, $\rho$ is the density, c is the specific heat, k is the thermal conductivity, and $\mathrm{\Delta }\mathrm{\ell }$ is a characteristic element length in the direction of flow. Large values of $\gamma$ indicate that convection dominates over diffusion on the spatial scale defined by the element size, $\mathrm{\Delta }\mathrm{\ell }$. 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.

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.

MASS FLOW RATE

MASS FLOW RATE, OP=MOD (default)

MASS FLOW RATE, OP=NEW

AMPLITUDE, NAME=name
MASS FLOW RATE, AMPLITUDE=name

MASS FLOW RATE, USER

MASS FLOW RATE, INPUT=file_name

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 in Abaqus/Standard for more information.

RADIATION VIEW FACTOR

HEAT TRANSFER, MXDEM=max_delta_emissivity

Step module: Create Step: General: Heat transfer: Incrementation: Max. allowable emissivity change per increment