ANSYS Fluent solves the energy equation in the following form:
(5–1) |
where is the effective conductivity (
, where
is the turbulent thermal conductivity, defined according to the turbulence model being used), and
is the diffusion flux of species
. The first three terms on the right-hand side of Equation 5–1 represent energy transfer due to conduction, species diffusion, and viscous dissipation, respectively.
includes volumetric heat sources that you have defined but not the heat sources generated by finite-rate volumetric or surface reactions since species formation enthalpy is already included in the total enthalpy calculation (see Equation 5–8).
In Equation 5–1,
(5–2) |
where sensible enthalpy is defined for ideal gases as
(5–3) |
and for incompressible flows as
(5–4) |
In Equation 5–3 and Equation 5–4, is the mass fraction of species
and
(5–5) |
The value used for in
the sensible enthalpy calculation depends on the solver and models
in use. For the pressure-based solver
is 298.15 K except for PDF models in which
case
is
a user input for the species. For the density-based solver
is 0 K except when modeling species transport
with reactions in which case
is
a user input for the species.
The energy equation is solved in moving (relative) frames of reference. In moving frames of reference, the energy transport equation uses rothalpy as a conservative quantity. See Equation 2–6 for the energy equation in moving frames of reference.
When the non-adiabatic non-premixed combustion model is enabled, ANSYS Fluent solves the total enthalpy form of the energy equation:
(5–6) |
Under the assumption that the Lewis number (Le) = 1, the conduction
and species diffusion terms combine to give the first term on the
right-hand side of the above equation while the contribution from
viscous dissipation appears in the non-conservative form as the second
term. The total enthalpy is defined as
(5–7) |
where is the mass fraction of species
and
(5–8) |
is the formation enthalpy of species
at the reference temperature
.
Equation 5–1 includes pressure work
and kinetic energy terms, which are often negligible in incompressible
flows. For this reason, the pressure-based solver by default does
not include the pressure work or kinetic energy when you are solving
incompressible flow. If you want to include these terms, use the define/models/energy? text command. When asked to include pressure work in energy equation? and include kinetic energy in energy equation?, respond
by entering yes in the console window.
Pressure work and kinetic energy are always accounted for when you are modeling compressible flow or using the density-based solver.
Equation 5–1 and Equation 5–6 describe the thermal energy created by viscous shear in the flow.
When the pressure-based solver is used, ANSYS Fluent’s default
form of the energy equation does not include them (because viscous
heating is often negligible). Viscous heating will be important when
the Brinkman number, , approaches or exceeds
unity, where
(5–9) |
and represents the temperature difference
in the system.
When your problem requires inclusion of the viscous dissipation
terms and you are using the pressure-based solver, you should enable
the terms using the Viscous Heating option in
the Viscous Model Dialog Box. Compressible flows typically have . Note, however, that when the pressure-based solver is used, ANSYS Fluent does
not automatically enable the viscous dissipation if you have defined
a compressible flow model.
When the density-based solver is used, the viscous dissipation terms are always included when the energy equation is solved.
Equation 5–1 and Equation 5–6 both include the effect of enthalpy transport due to species diffusion.
When the pressure-based solver is used, the term
is included in Equation 5–1 by default. If you do not want to include it, you can disable the Diffusion Energy Source option in the Species Model Dialog Box.
When the non-adiabatic non-premixed combustion model is being used, this term does not explicitly appear in the energy equation, because it is included in the first term on the right-hand side of Equation 5–6.
When the density-based solver is used, this term is always included in the energy equation.
Sources of energy, , in Equation 5–1 include the source of energy due to
chemical reaction:
(5–10) |
where is the enthalpy of
formation of species
and
is
the volumetric rate of creation of species
.
In the energy equation used for non-adiabatic non-premixed combustion
(Equation 5–6), the heat of formation is included
in the definition of enthalpy (see Equation 5–7), so reaction sources of energy are not included in .
When one of the radiation models is being used, in Equation 5–1 or Equation 5–6 also includes radiation source terms. For details, see Modeling Radiation.
When the electric potential equation Equation 20–1 is being solved, in Equation 5–1 also includes
Joule heating source terms.
It should be noted that the energy sources, , also include
heat transfer between the continuous and the discrete phase. This
is further discussed in Coupling Between the Discrete and Continuous Phases.
In solid regions, the energy transport equation used by ANSYS Fluent has the following form:
(5–11) |
|
where | |
|
| |
|
| |
|
| |
|
| |
|
|
The second term on the left-hand side of Equation 5–11 represents convective energy transfer
due to rotational or translational motion of the solids. The velocity
field is computed from the motion specified for the solid zone. (For details,
see Solid Conditions in the User's Guide). The terms on the right-hand side of Equation 5–11 are the heat flux due to conduction
and volumetric heat sources within the solid, respectively.
When you use the pressure-based solver, ANSYS Fluent allows you to specify anisotropic conductivity for solid materials. The conduction term for an anisotropic solid has the form
(5–12) |
where is the conductivity
matrix. See Anisotropic Thermal Conductivity for Solids in the User's
Guide for details on specifying anisotropic conductivity
for solid materials.
The net transport of energy at inlets consists of both the convection and diffusion components. The convection component is fixed by the inlet temperature specified by you. The diffusion component, however, depends on the gradient of the computed temperature field. Thus the diffusion component (and therefore the net inlet transport) is not specified a priori.
In some cases, you may want to specify the net inlet transport
of energy rather than the inlet temperature. If you are using the
pressure-based solver, you can do this by disabling inlet energy diffusion.
By default, ANSYS Fluent includes the diffusion flux of energy at
inlets. To turn off inlet diffusion, use the define/models/energy? text command and respond no when asked
to Include diffusion at inlets?
Inlet diffusion cannot be turned off if you are using the density-based solver.