Hello and Welcome,
The Solution tab of Ansys Fluent has options that can be used
to control and monitor the solution of a CFD simulation.
Before starting any CFD simulation, the solution needs to be initialized,
i.e., a starting guess value of the solution variables need to be
imposed onto the computational mesh, and
only then should the solver be triggered to run the simulation.
The focus of this video is on the different types of initialization methods
available in Ansys Fluent.
Let’s get started.
Ansys Fluent solves various governing equations iteratively
to calculate the solution.
However, before starting any simulation, Fluent requires
the solution variables to be initialized.
Initialization primarily means that every individual cell must be assigned
a value for every solution variable
to serve as an initial guess for the solution.
The general parameters that are considered for initialization are
pressure, velocity, temperature - if energy equation is turned on,
and turbulence parameters based on the turbulence model used.
For more information on initialization parameters for
different physics models, refer to Fluent User Guide.
A more realistic initial guess improves stability
and accelerates convergence.
There are five different ways to initialize a solution in Fluent
1. Standard initialization 2. Hybrid initialization
3. FMG initialization 4. Starting from a Previous Solution and 5. Patching.
Hybrid initialization is the default method Fluent uses
and is recommended for most of the cases.
Let us look at the differences between various initialization methods through an example.
We will consider the initialized flow-field
for the case of a flow past a cylinder.
Standard initialization takes the values defined by the user
for the solution variables and initializes the flow field to these values.
As you can see here, constant values of velocity have been initialized
in the computational domain.
Here, the values can be entered manually, computed from information
based on a specified zone, or averaged based on all zones.
Though not the default initialization method, this is the recommended
approach for advanced simulations such as those involving porous media.
Hybrid on the other hand, provides a slightly more realistic approach
by imposing a non-uniform initial guess,
which is evident from the contours shown here.
In this method, a Laplace equation is solved to determine the velocity
and pressure fields, and all other variables are automatically patched,
based on domain-averaged values or a predetermined interpolation approach.
This is the default initialization method in Ansys Fluent
and works well for a wide range of problems.
Full Multi Grid, also known as FMG initialization method
provides much more realistic non-uniform initial values
as seen from the contours.
It is an advanced initialization technique that is called through
a text-based command.
Here, inviscid Euler equations are solved by automatically constructing
a desirable number of geometric grid levels.
For more information on this approach, please refer to the User’s Guide.
Though FMG takes slightly longer than other methods,
a good initial solution can be obtained
in a fraction of the time spent to converge on a final solution.
This method could be beneficial for simulations involving
compressible flows and rotating machinery.
It should be noted that in general, the closer the initial guess
is to the final solution, the faster is the convergence.
From the examples, it is evident that the FMG initialization method
provides a more realistic initial guess to the actual solution.
Hybrid on the other hand, provides a slightly less realistic initial guess than
FMG, but better than the standard initialization method.
Now let us look at the process of initializing the solution using common initialization methods,
i.e., hybrid and standard through an example.
We will also demo the patching method, which can be used in
conjunction with other initialization methods if required.
Launch Ansys Fluent in solution mode.
Go to File and read the case file of a “mixing-tee” model
which contains both solid and fluid domains.
The computational model setup is already completed in Ansys Fluent.
Now, let us directly proceed to look at how different initialization
methods can be employed here.
Go to the Solution tab. Note that the Solution tab can be accessed from
the Ribbon as well as from the tree in the Outline View.
By default, hybrid initialization is selected in Fluent, which is also
generally recommended for all single-phase steady-state flows.
When the Initialize button is clicked, the solver initializes the solution
after solving the Laplace equation for 10 iterations to
setup the pressure and velocity fields.
The residuals of the solution for these 10 iterations
are printed in the console window.
For most cases 10 iterations are sufficient, however
the number of iterations can be changed by specifying the
number of iterations in More Settings if required.
Let us use the same problem again,
but now we will perform the standard initialization.
To employ this method, select Standard from Method
in the Initialization group, and click on Options
to view and edit the initialization values.
In the drop-down menu available, you can choose a surface from
which the values for the parameters should be taken from.
You can also select all-zones to compute average values based
on all zones or enter the values manually for
each parameter to which you want the flow field to be initialized.
Once selected, the parameter values will be automatically displayed
in the Initial Values. Click on Initialize to initialize the solution.
To compare both hybrid and standard initialization methods visually,
let us look at the velocity contours for both.
As seen from the image on the left, the standard initialization
will initialize the entire flow field with a single value.
Whereas the hybrid initialization on the other hand initializes the flow field
with spatially varying values making it more realistic to the actual solution.
Let us now look at the next method of initialization, i.e., patching.
The patch option is used to patch different values of flow variables onto different cells.
You can patch constant values, custom field functions or expressions
to cell zones and cell registers.
The patch operation is widely used in Multiphase flows.
Now let’s go ahead and see how the patch option works.
As mentioned earlier, patching can be performed alongside
other initializations in a similar manner.
So, let us continue with the case where we already performed
the standard initialization.
The goal now is to patch a temperature value of a 100 degrees Celsius onto the solid pipe.
To perform the patch operation, click on the Patch option
and select the variable to be patched,
which is temperature and then select the zone that needs to be patched
with the selected variable.
Also define the temperature value to which the solid pipe is to be patched;
here it is a 100 degrees Celsius.
Click on patch and close the dialog box.
You can now see that the solid wall is patched with a temperature
of a 100 degrees Celsius.
To get a clear picture of how the standard and the hybrid initialization methods compare to the final solution,
To get a clear picture of how the standard and the hybrid initialization
methods compare to the final solution,
let us look the velocity contours before
and after the simulation is completed.
Here it is evident that the hybrid initialization
provides closer initial guess to the solution
than the standard initialization.
Let us now summarize what we learned in this video.
We discussed the importance of initialization and the impact of
various available initialization methods in Ansys Fluent through an example.
We also looked on how to employ the standard, hybrid, and patch
initialization methods using a hands-on demo.
This brings us to the end of our video.
Thank you very much for watching.