The procedure for setting up a heat transfer problem is described below.
Create a sub-task for the heat transfer problem.
Create a sub-task
Select the appropriate problem type from the Create a sub-task menu.
For heat transfer in a solid region, select Heat conduction problem.
Heat conduction problem
For a nonisothermal flow problem, select one of the following, depending on the type of flow being modeled:
Generalized Newtonian non-isothermal flow
problem
Differential viscoelastic non-isothermal flow
problem
Integral viscoelastic non-isothermal flow
problem
Darcy non-isothermal flow problem
Film model: Gen. Newtonian
non-isothermal
Film model: Viscoelastic
non-isothermal
Shell model: Gen. Newtonian
non-isothermal
Shell model: Viscoelastic
non-isothermal
When prompted, specify a name for the sub-task.
Specify the region where the sub-task applies.
Domain of the sub-task
Define the material properties.
Material data
For a simple heat conduction problem, the material data that must be entered are the thermal conductivity (
in Equation 13–2) and the heat source per unit volume
(
in Equation 13–1).
Thermal conductivity
Heat source per unit volume
The other quantities can be discarded.
For a general heat transport problem, in other words, including rigid body motion of a solid and/or transient, you will also need to define the specific heat capacity and the density (C
and 
in Equation 13–4):
Heat capacity per unit mass
Density
When a rigid body motion is involved, you will need to define the translation velocity (see below).
In addition, an average temperature can be entered to facilitate convergence in nonlinear problems.
Average temperature
The closer this temperature is to the solution, the better the convergence will be. If this temperature is too far from the solution, the numerical scheme might diverge. Note that, for time-dependent problems, this value is used as an initial temperature condition.
For a nonisothermal flow problem, in addition to the flow properties (for example, viscosity and density), you will need to define the thermal conductivity (
in Equation 13–2) and the specific heat capacity and
heat source per unit volume (
and 
, respectively, in Equation 13–5.
Thermal conductivity
Heat capacity per unit mass
Heat source per unit volume
By default, viscous and wall friction heating (or dissipation) is neglected in the energy equation. For some nonisothermal flows, it is preferable to solve the flow first without viscous and wall friction heating, then add viscous and wall friction heating and continue the calculation. To add viscous and wall friction heating to the energy equation, select Viscous (+ Wall friction) heating and choose the Viscous + wall friction heating will be taken into account menu item.
Viscous (+ Wall friction) heating
If you choose to use the Boussinesq approximation for density (see Boussinesq Approximation for Density in Nonisothermal Flows), you will need to specify the thermal expansion coefficient (
in Equation 13–9).
Coefficient of thermal expansion
You will also be prompted here to enter the reference temperature (
in Equation 13–9). Important: For information about setting other flow properties (such as viscosity), see the procedure for the type of flow you are modeling (Problem Setup for generalized Newtonian flow, Problem Setup for Differential Viscoelastic Flows for differential viscoelastic flow, Problem Setup for Integral Viscoelastic Flows for integral viscoelastic flow).
Define the flow boundary conditions (nonisothermal flows only).
Flow boundary conditions
See the procedure for the type of flow you are modeling (Problem Setup for generalized Newtonian flow, Problem Setup for Differential Viscoelastic Flows for differential viscoelastic flow, Problem Setup for Integral Viscoelastic Flows for integral viscoelastic flow) for details about setting flow boundary conditions.
Define the thermal boundary conditions.
Thermal boundary conditions
Select the boundary for which you want to set thermal conditions.
Click Modify.
Select the boundary condition type you want to impose. For each external boundary, there are four possible conditions for a heat conduction problem, and five or six for a nonisothermal flow. For interface boundaries, the temperature and heat flux can be continuous or discontinuous across the boundary. By default, Ansys Polydata imposes a zero temperature on all external boundaries, and continuous temperature and heat flux across interfaces.
Choose Temperature imposed to specify the temperature on the boundary.
Temperature imposed
Select the appropriate specification method:
Select Constant to set a constant value for temperature.
Select Linear function of coordinates to specify a linear function of the form
for the temperature. Select Map from CSV (Excel) file to impose a temperature profile contained in a CSV file. Note that boundary conditions imposed via a CSV file are evaluated only once. In other words, if the CSV file contains a temperature distribution in space, the evaluation will be based on the geometry that is known at the beginning of the calculation, even if the boundary is moving.
Select User-defined function to impose a temperature profile using a UDF.
Choose Flux density imposed to specify the heat flux on the boundary.
Flux density imposed
The inputs are
(which can be constant or a linear
function of the form 
), 
, 
, 
, 
, and 
in Equation 13–7. To specify 
as an absolute temperature, set the
reference temperature 
to 0. Otherwise, set 
to the appropriate reference
temperature and then specify 
relative to 
. For example, to work in degrees
Celsius, 
should be equal to 273.15;
is the ambient temperature. Note that
and 
do not need to be the same. For
example, radiation may be controlled by a far-field
temperature 
, while natural convection occurs at
the boundary with a fluid whose temperature is different
from the far-field temperature. Since the Stefan-Boltzmann Law is a nonlinear function of temperature, it may require an evolution scheme. In this case, you can define an evolution scheme on the ambient temperature
in such a way that 
changes progressively from the average
temperature to its actual value. See Evolution.Choose Insulated boundary / symmetry to specify an insulated boundary.
Insulated boundary / symmetry
No further inputs are required.
Choose Inflow (available only for nonisothermal flows when the same boundary has been defined as an inflow boundary in the Flow boundary conditions menu) to assign a fully-developed inlet temperature profile for the boundary.
Inflow
Ansys Polyflow will compute the profile automatically, so no further inputs are required.
Choose Outflow (available for nonisothermal flow only; not available for heat conduction problems) for a vanishing conductive heat flux.
Outflow
No further inputs are required.
Choose Rosseland Correction to use the Rosseland approximation for radiative heat transfer.
Rosseland Correction
This option is used primarily in glass melting problems. See Radiative (Rosseland) Correction for details. Note that the Rosseland approximation is a more computationally inexpensive alternative to the use of an internal radiation sub-task (as described in Internal Radiation), and should not be invoked for boundaries of a domain in which an internal radiation sub-task is defined.
Choose Inlet of periodic condition to specify a periodic boundary for a periodic heat transfer problem.
Inlet of periodic condition
Periodic boundary conditions are used when the physical geometry of interest and the expected temperature-field pattern have a periodically repeating nature. This means that the heat fluxes across two opposite planes in your computational model are identical. Periodic boundary conditions can be applied to a pair of boundary sections, which are referred to as the inlet and outlet of the periodic condition. The temperature field and heat flux are continuous between the inlet and outlet.
The inputs for the periodic inlet are as follows:
In the resulting Inlet of periodic cond. panel, select the corresponding periodic boundary section (the outlet of the periodic condition) and click Select.
Specify the transformation of coordinates and temperature field on the inlet to those along the outlet. There are two ways to do this:
Specify a rotation matrix and/or translation vector explicitly. For rotational periodicity, specify the rotation matrix.
Direct modification of rotation
matrix
For translational periodicity, specify the translation vector.
Direct modification of translation
vector
The rotation matrix and/or translation vector, once applied to the coordinates of a node along the inlet, will produce the coordinates of the corresponding node along the outlet.
Specify pairs of corresponding points on the inlet and outlet: two points on the inlet and two points on the outlet for 2D, or three points on the inlet and three points on the outlet for 3D.
Definition by source-target
points
Ansys Polyflow will determine the proper rotation matrix and translation vector based on these sets of points, and then apply it to the rest of the points on the inlet to obtain the points on the outlet.
Note that, for axisymmetric problems, only translations along the
axis are allowed; no rotation or
other translations are possible. Check the transformation to be sure it is consistent with the mesh.
Test of the transformation
When you are satisfied with the inputs, accept the settings.
Accept current parameters
Specify the difference in heat flux between the inlet and the outlet.
Note that there are no inputs for the outlet of the periodic condition.
Choose Source of the connected condition to specify the "source" boundary in a pair of non-conformal boundaries that need to be connected.
Source of the connected condition
Non-conformal boundary conditions are described in Non-Conformal Boundaries. The inputs for non-conformal thermal boundary conditions are the same as those for flow boundary conditions, as described in Connecting Non-Conformal Boundaries, except for the numerical parameters. The first two numerical parameters (element dilatation and amplitude of volume generation) are the same as for flow boundary conditions, but the stabilization factor for flow conditions is replaced by a smoothing factor for thermal conditions.
The smoothing factor controls the amount of heat flux that is allowed to be conducted through faces that are connected to only one of the connected boundaries (that is, just to the source boundary or just to the target boundary). Ideally, there should be no conductive heat loss through these faces. The smoothing factor is therefore set to a very large value (causing the faces to become insulated walls with a uniform temperature), to avoid conductive heat loss.
Important: Changing the value of the smoothing factor from the default value is not recommended, except on the advice of your support engineer. Note that setting this value to zero will destabilize the solution.
Choose Interface (available only for interfaces between subdomains) to indicate whether the heat flux across the boundary should be continuous or discontinuous. (The temperature across the boundary is always continuous.)
Interface
By default, the heat flux is continuous. To specify discontinuous heat flux across the interface, you can define a nonzero value for the heat flux jump
, which is computed the same way
is computed in Equation 13–7.
This can be used, for example, to simulate internal
radiation. The inputs for a nonzero 
are the same as those listed above for
the Flux density imposed condition.
You can choose Incoming fluid temperature for boundaries that experience both incoming and outgoing flows (for example, outlets of the flow domain through which some fluid enters as backflow). This option is only available for nonisothermal flow simulations, and imposes a temperature on the flow that enters the domain in order to maintain the stability of the simulation (as described in Boundaries with Incoming and Outgoing Flows).
Incoming fluid temperature
In the menu that opens, you can set parameters used in Equation 13–10: the imposed temperature (
), the minimum normal velocity
(
), and the penalty coefficient
(
).A local temperature will be applied to the nodes of the boundary where the local normal velocity of the flow entering the domain is greater than or equal to the specified minimum normal velocity. Note the following when setting the parameters:
It is necessary to set
to a value that is greater than
zero, in order to avoid a conflict with the
boundary condition of the boundary. In general, it
is recommended that you set 
to a very small value relative
to the dimension scale of your problem, so that it
is close to zero; however, if you have concerns
about either the assumptions inherent in
simulating backflow or the results that you are
obtaining, you have the option of setting
to the highest velocity that yet
produces a stable calculation, therefore
minimizing the extent of the incoming flow on
which temperatures are imposed.The local temperature is calculated via a penalty formulation, so higher values for the penalty coefficient cause the local temperature to be closer to your specified imposed temperature. Note that if the penalty coefficient is too high, the simulation can become unstable. For this reason, it is recommended that you apply evolution on the penalty coefficient.
Applying evolution on the parameter(s) generating the incoming flow can be helpful.
For more information on setting boundary conditions, see Boundary Conditions.
(optional) Modify the interpolation scheme for temperature.
Interpolation
See Interpolation for Nonisothermal Flows for interpolation guidelines for generalized Newtonian nonisothermal flows. (These guidelines apply to differential viscoelastic flow as well. For integral viscoelastic flow, you will not be able to modify the interpolation scheme for temperature.)
It is also possible to define different interpolation types for temperature in different parts of the domain of the sub-task:
Select Sub-interpolation at the bottom of the Interpolation menu.
Sub-interpolation
In the Sub-interpolation menu, select the subdomain on which you want to modify the interpolation
Choose the type of interpolation you want on this subdomain.
Ansys Polyflow will automatically apply conformity constraints, so as to maintain the continuity of the temperature field across the interface together with continuity of the heat flux.
Subdivided elements are mostly useful for solving flow problems in which advection takes place.
(optional) Specify the transport velocity.
Transport velocity
For a general heat transport problem, in other words, including rigid body motion of a solid, you will also need to define the transport velocity.
First, you must select
Modify status = .FALSE.
for it to become active (TRUE).
Then enter the non-zero component(s) of the translation velocity of the solid body
Modify vtransx = 0.0000000E+00
Modify vtransy = 0.0000000E+00
Modify vtransz = 0.0000000E+00
When modeling heat conduction in a solid, problems are usually linear and so it is generally not necessary to use an evolution scheme. Nonlinearities arise when a nonlinear temperature law is used for the conductivity or when radiation boundary conditions are used.
If there are convergence difficulties related to radiation, the use of an
evolution scheme that increments the reference temperature 
with the evolution parameter 
is recommended. See Evolution for
information on evolution. Note that a convective term defined in a boundary
condition does not make the problem nonlinear.
See Using Evolution to Compute Generalized Newtonian Flow for suggestions on using evolution for generalized Newtonian nonisothermal flow calculations. These guidelines are also appropriate for other types of flow.
As with all nonlinear problems, you may encounter some convergence difficulties. For nonisothermal flows, these difficulties are often attributable to the combination of viscous and wall friction heating, thermal convection, and the temperature dependence of the viscosity. You can try to improve convergence by applying evolution as part of your nonisothermal simulation. An easy way to do this is available for tasks defined as Steady or Evolution problem(s): simply click Enable convergence strategy for thermal flows in the Numerical parameters menu. Note that the current task will then be converted into an evolution task if it was previously defined as a steady task. This strategy can be combined with the convergence strategy for rheology/slip.
When this option is enabled, the viscous and wall friction heating, thermal convection, and temperature dependence of the viscosity is progressively introduced into the system of equations being solved over the course of multiple evolution steps. A linearly increasing evolution function is defined for the viscous and wall friction heating and for the temperature dependence of the viscosity; at the same time, a linearly decreasing evolution function is defined for the thermal conductivity. More precisely:
The linearly increasing evolution function starts at 0 and is incremented up to 1. When the evolution function is 0, the viscous and wall friction heating and temperature dependence of the viscosity are discarded, whereas they are fully incorporated into the equations when the evolution function is 1.
The linearly decreasing evolution function applied to the thermal conductivity starts at 1000 and decreases down to 1. When it equals 1000, heat transfer is dominated by conduction, whereas convection is fully incorporated into the equations when the evolution function equals 1.
Note that when you use the Enable convergence strategy for thermal flows menu item to "automatically" define the evolution, it is not necessary to "manually" define the previously mentioned evolutions using the button and the items in the Material Data menu. If an evolution function is manually defined on a parameter that is affected by the automatic evolution definition (that is, viscous and wall friction heating, thermal conduction, and the temperature dependence of the viscosity), such a manual definition will be ignored during the calculation and the automatic definition will prevail.
This convergence strategy is available for all nonisothermal flows that obey generalized Newtonian or differential viscoelastic laws, though it is not mandatory. If you do not enable evolution for nonisothermal flows, a window will open at the end of your session to verify that this was intentional: it will inform you that nonisothermal flows can cause convergence difficulties, and ask whether you want to activate the convergence strategy. If you click , the evolution for nonisothermal flows will be enabled with the functions described previously.
The aim of the convergence strategy is to facilitate the start of the calculation, and in no way will it guarantee that a solution will be obtained for every case. It is important to note that the evolution for nonisothermal flows takes care of the nonisothermal component of the flow case only. In other words, it is always a good idea to make sure that the corresponding isothermal calculation converges. When necessary, the convergence strategy for non-isothermal flows can be combined with the convergence strategy for rheology and slipping (see Convergence Strategy for Rheology and Slipping).
While this convergence strategy is expected to lead to a solution in most cases, it by no means provides the optimum solution settings in terms of solution speed. Other solution setups may be found that result in a faster solution; you should investigate such solution setups on a case-by-case basis.