When you solve a heat transfer problem
in Fluent,
you have to specify
thermal boundary conditions
for all flow boundaries
and all walls.
Flow boundaries are easy –
just go to the thermal tab
in the boundary conditions panel
and enter the temperature.
At inlets,
this is obviously just the temperature of the fluid
as it enters the domain.
At outlets,
the value you enter is the
backflow temperature and Fluent will only use it
if there is reverse flow,
and then only at parts of the boundary
where reverse flow actually enters the domain.
If there is no reverse flow,
the backflow value will not have
any effect on the solution,
but it is usually a good idea
to enter a reasonable value
in case reverse flow occurs
during part of the iterative process.
Now let’s look at the
boundary conditions panel for a wall.
The default condition for a wall
is constant heat flux
with a value of zero,
which would mean there is no heat transfer
through the wall.
We call this an adiabatic boundary condition.
If you want to have heat transfer,
then you can enter a non-zero value
for the heat flux,
or you can set the wall temperature.
The basic idea is that
if you define the heat flux,
then your CFD calculation will calculate
what the wall temperature has to be
in order to achieve that heat flux,
or conversely,
if you define the temperature,
Fluent will calculate
what the heat flux is for that temperature.
Sometimes, there might be uncertainty
about conditions right at the wall,
but if you know how the wall exchanges heat
with the environment outside the domain,
you can use convection, radiation
or mixed conditions.
In the convection BC,
you enter the value for the
free stream temperature
and the heat transfer coefficient.
These represent the temperature
of the environment outside
of the computational domain
and the heat transfer coefficient
between the wall and its environment.
So basically,
the heat flux through the wall is a function
both of the inputs in the panel
and the calculated wall temperature
at the current iteration.
The radiation boundary condition is similar,
except now heat transfer
between the wall and the environment
occurs by means of radiation,
and if you select Mixed, then
both convection and radiation are included.
The other options are used
only in special cases.
Via System coupling is used for certain
thermal fluid structure interaction problems,
and via Mapped Interfaces
is used with certain kinds of
non-conformal mesh interfaces.
If your model includes both solid zones
and fluid zones,
like the one here on the screen
then you are solving what is called
a conjugate heat transfer problem.
It is called conjugate heat transfer,
because at the wall,
convection from the fluid to the wall
is coupled to conduction
from the wall into the solid.
Or vice versa
if the solid is warmer than the fluid.
In conjugate heat transfer problems,
when Fluent first loads the mesh,
it makes an identical copy
of the wall of the solid.
This copy is known as a shadow wall,
so you can see here in the panel
there is a wall-coil
and a wall-coil-shadow.
One side of the wall and wall shadow pair
is attached to the fluid zone,
and the other side will be
attached to the solid zone.
You can see which one is which
by looking in the Adjacent Cell Zone field.
For a conjugate heat transfer problem,
the boundary condition used at the Wall
is the coupled boundary condition.
This means that at every mesh face on a wall,
the temperature at the corresponding
mesh face on the shadow wall is identical,
and heat fluxes are equal and opposite.
It is possible to break the thermal coupling
between the wall and its shadow
by selecting heat flux or temperature,
but there are few, if any, circumstances
where it would be physically meaningful
to do so and it would also no longer
be a conjugate heat transfer model
because the heat transfer in the fluid would be
independent of the heat transfer in the solid.
One additional thing I want to talk about
is energy sources.
It is not unusual for heat transfer problems
to make use of energy sources, for instance
to represent the heat generated by
an electrical component.
In the model on the screen now,
the coil is made out of copper
and it is heated by electrical resistance.
To simplify the modeling,
the heating is represented
as a uniform volumetric energy source.
To define this source,
just open the cell zone conditions panel
for the solid, go to the sources tab
enter one or more sources
and then enter values.
The units of the source term
are power per unit volume,
so if you are using SI units,
energy source terms usually have large values.
When the value used here
is multiplied by the volume of the coil,
the total energy source term
turns out to be 2.9 megawatts,
and remember if you need to find the volume
of your solid zone, you can use
the volume integrals panel to do that.
Even though this model
only has an energy source in the solid,
there can also be sources in the fluid,
and while we have used a constant value
in this problem,
it is also possible to use profiles,
or user-defined functions,
or expressions
to make the source term non-uniform,
and/or a function of other solution variables.
Before moving on to the next topic,
I just want to summarize the main steps
for setting thermal boundary conditions:
At flow inlets and flow outlets,
you have to define the temperature
and the values at outlets only apply
when reverse flow enters your domain.
At walls,
there are a number of different possibilities
and you can choose the one
that best matches your problem.
If you have conjugate heat transfer,
keep the setting of coupled
for the thermal boundary condition
on walls with shadows.
And, you also have the option
to define volumetric energy sources
in both solid cell zones and fluid cell zones.