Welcome to this Ansys How-To Series video.
We know that heat transfers by three modes: conduction, convection, and radiation.
Here, let’s have a look at convection specifically. Convection occurs in fluids, which are liquids
and gases. In engineering, we can find convection occurring
in so many situations. For example, heat released from the chimney
of a factory to the air, heat dissipated from hot devices to the ambient like integrated circuits.
So, convection is an important boundary condition
in almost every thermal analysis.
When dealing with Convection, the film coefficient, also known as the heat transfer coefficient,
plays an important role. The film coefficient can be thought of as
the amount of heat flux needed to cause a unit difference in temperature between the
surface and the ambient temperature. Although the film coefficient may be dependent
on many factors, having a temperature-dependent film coefficient is common in thermal analyses.
Therefore, in this video, we will introduce how to define temperature-dependent film coefficients.
In fact, convection is a very complex process. It includes sub-mechanisms of advection and diffusion.
Advection describes the transport of substance
by bulk motion. And diffusion describes the transfer of substance
due to heat gradients. In the simulation, convection can be solved
in two ways. One way is to use Computational Fluid Dynamics Solver.
It solves fluid flow and energy equation in
the fluids, as well as in the solids.
The other way is to include convection within a conduction-based solver.
It is a simplified method that treats convection as a boundary condition controlled by two
parameters - film coefficient, and bulk temperature.
The convection heat transfer is described by this equation, where ‘Q’ is the heat
transfer rate caused by convection, ‘h’ is the film coefficient, ‘A’ is the area
of the body in contact with the fluid, ‘Ts’ is the surface temperature, and ‘Tb’ is
the bulk fluid temperature.
For example, here we have a hot CPU with a heat sink dissipating heat to the air.
Then ‘Ts’ is the temperature of the heat sink surfaces, ‘Tb’ is the temperature
of the fluid, which is the ambient air. And ‘A’ is the area of the heat sink surfaces
exposed to air.
Now you can understand why heat sink is always designed with so many fins.
Basically, with increased exposed areas of the fins, heat can be dissipated more efficiently
by convection.
Now let’s focus on film coefficient ‘h’. The film coefficient can be dependent on various
physical variables, like Fluids Property, Fluid Velocity, Geometry Shape & Orientation,
Surface Roughness, and Temperature, etc. Note that the film coefficient ‘h’ does
not have to be constant. In Ansys, ‘h’ can be defined as a constant,
a function, or a tabular input. And it can be defined as spatial-dependent,
time-dependent, or temperature-dependent.
As we mentioned before, the temperature-dependent film coefficient is common in thermal analyses,
so we will focus on how to define temperature-dependent film coefficient by tabular input.
Note that by saying the film coefficient is “temperature-dependent”, ‘h’ can be
controlled by the temperature of the surface, the temperature difference of the surface
and the bulk temperature, or the average temperature of the surface and the bulk temperature.
In short, flexibility is provided on which 'temperature' we want to make the film coefficient
depend on.
Now let’s use a simple example to show you how to define temperature-dependent film coefficient
in Ansys simulation.
For this case, we have a simple plate of Structural Steel.
Let us perform a Transient Thermal Analysis on this case.
The plate is meshed with default mesh settings. Now, let us apply a Temperature of 100 degrees
Celsius on a side of this plate. And solve the case for this temperature gradient.
Alright, now right-mouse-click on Solution and insert Temperature result.
Evaluate the Results to check the temperature plot.
As the initial temperature is 22 degrees Celsius, we can see the temperature gradient from 22
degrees Celsius to 100 degrees Celsius.
Now, let us add the Convection boundary condition to this plate.
For this conduction-based solver, it will be treated as a boundary condition driven
by two parameters - film coefficient and bulk temperature.
Here, we can add Convection by right-mouse-clicking on Transient Thermal and inserting Convection.
Select the upper face to assign the Convection boundary condition.
Note that we need to select the faces that are exposed to the surrounding fluid, such
as liquids or gases.
Under the Convection definition, we can define the Film Coefficient using three methods – Constant,
Tabular Data, and Function. Using the Constant option, we can define the
constant film coefficient over the surface. But if we have varying film coefficients then
we can use either Tabular Data or Function option.
For example, when using the Function option, we can define the film coefficient to be a
function of a variable – such as time. For that, you can simply insert the expression
in the input field like this. Additionally, we can also import Time-Dependent
or Temperature-Dependent external data as well.
First, let us define a constant film coefficient and run the case to observe the results.
Then, in the second case, let us use Tabular Data for defining Temperature-Dependent Film Coefficient.
So, let us select the Tabular Data input under
the Convection boundary condition. Now, select Temperature as the Independent Variable.
For Coefficient Type, select Average Film
Temperature, which means we will evaluate the film coefficient at the average value
of Surface Temperature and Bulk Temperature. Now, enter the temperature-dependent convection
coefficient in the table. If required, you can add more temperature-dependent
film coefficient values in the table.
Now, let us solve the case and observe the results on the Temperature plot.
Comparing the results, we can see the difference in temperature plots for the constant film
coefficient versus the temperature-dependent film coefficient based boundary conditions.
The result of the film coefficient is not directly available.
We need to use the User Defined Result. But for that, we need to first understand,
how the convection boundary condition is applied in the solver.
For the faces, selected for convection boundary condition, the solver creates surface elements
for 3D thermal surface effect – namely SURF152. Thus, we need to first extract these SURF152
elements and then extract the film coefficient on those elements using the NMISC5 variable.
So, select Worksheet from the ribbon under Solution, and select Material and Element
Type Information. Here, select SURF152 and right-mouse-click
to Create User Defined Result. A new User Defined Result is added to the tree.
For this result, we can define Expression
as NMISC5 to extract the convective film coefficient. Then, evaluate the results.
We can see the contour plot for the film coefficient and how it varies with time.
Now, let us add the similar User Defined Result for the other case of constant film coefficient.
And we can see that it is constant through the solution time.
To summarize, convection is a complex process. In conduction-based solver, convection is
simplified and is treated as a boundary condition controlled by two parameters - film coefficient
and bulk temperature. The film coefficient is dependent on various
physical variables and is usually empirically obtained.
In the thermal analysis, it’s very common to see the temperature-dependent film coefficient.
Ansys provides a simple way to input the film coefficient as tabular data that varies with temperature.
And we can visualize the distribution of film
coefficient in post-processing.
If you find this video helpful, please like, comment, and subscribe. To find more information
about thermal analysis or similar topics, check out our channel for more how to videos
and visit ansys.com/courses today!