Hello and Welcome!
When performing simulations
using Ansys Fluent,
once the Numerical Mesh is loaded
and all the necessary physics models
and boundary conditions have been defined,
we need to select the numerical schemes
and the solution controls
which Ansys Fluent Solver is going to use
for solving the CFD problem.
These options are contained in the Solution tab.
In addition to selecting the numerical methods
and solution controls,
other options available in this tab
can also help us
impose convergence conditions
by defining residuals and monitors,
select the way in which the flow field is initialized,
make the necessary final checks,
and run the simulation.
In this video
we will learn about the Solution Methods group
of the Solution tab.
More specifically,
we will learn about the
pressure-velocity coupling schemes
and the spatial discretization methods
used with the default
Ansys Fluent pressure-based solver.
Let's get started.
Here I have opened
an Ansys Fluent case file
in which physics have already been set.
Let us now directly go to the solution tab
which is located between the User-Defined tab
and the Results tab in the Ribbon.
The first group of the Solution Tab
is the Solution Methods group.
Clicking on the Methods options
opens the Solution Methods task page.
The focus of this course
will be the settings in this task page.
Ansys Fluent can simulate both
compressible and incompressible fluid flows
using two different solvers
The Pressure-based solver
and the Density-based solver.
For more details on specifics of these solvers,
you can refer to the lesson on physics tab
and also the Ansys Fluent user guide.
The Solution Methods task page
looks very different for the two different solvers.
As the Pressure-based solver is the most
commonly used flow solver,
and is the default option,
in this lesson we will discuss the various
options pertinent to the Pressure-based solver.
In the Solution Methods task page,
we can specify the inputs
for the Pressure-velocity coupling schemes,
flux types and different discretization methods
for the convective terms of the flow equations.
The default settings are recommended for most cases.
If you have experimented with various settings
and you would like to revert to the defaults,
you can always do this by clicking here on
Default.
Let’s now look
at the different available options
Let's start with
Pressure Velocity coupling Schemes.
These coupling schemes control the manner
in which the pressure and velocity fields
are updated when the pressure-based solver is used.
They can be either of the segregated type,
i.e., pressure and velocity are
updated sequentially such as
SIMPLE, SIMPLEC and PISO,
or coupled
where pressure and velocity are updated
simultaneously.
These 4 Pressure-Velocity Coupling methods,
available in Ansys Fluent,
can be selected from the dropdown menu here.
The default option, i.e., coupled,
is recommended for most steady-state flows.
In general,
segregated methods are faster per iteration,
while the coupled algorithm
usually requires fewer iterations to converge.
As coupled is default and applicable
to most simulation problems,
let's discuss the Coupled method further.
Coupled can be used with or without
the pseudo time method option,
which is a form of implicit under-relaxation,
and can be selected using this drop down
here further down in the task page.
The default is to use them together,
and the combination is often referred to
as the pseudo-transient solver.
Pseudo-transient is very robust
for most of the routine applications,
both compressible and incompressible.
When we use the pseudo-transient solver,
we will see an entry in the ribbon
for a Timescale Factor,
and it's useful to know what this does.
In the pseudo-transient method,
the Fluent solver advances the solution
from one iteration to the next by
using a false time step.
After enough iterations,
or false time steps
the solution will converge to a steady state flow.
The pseudo-time step size
is determined automatically by the solver,
based on characteristics of the
problem you are solving.
Please refer to the last lesson of this course
for more details
on the impact of the time scale factor.
You can also refer to the user
and theory guides for more specific
information about the method.
Let’s now discuss the inputs under spatial
discretization.
Here
we have options for the calculation
of the gradients and the advection terms
for all equations.
Note that the equation names
and the number of equations displayed here
depend on the physics models
chosen for the simulation.
For example, if energy is unchecked,
the energy equation option is not displayed
under spatial discretization.
Similarly,
if a different turbulence model is used,
variable names pertaining to that model are displayed.
The default values are highly recommended,
which are the least squares cell-based method
for the gradient,
the second order method for pressure
and the second order upwind
for all transport equations.
One notable exception applies though
to pressure discretization
Although second order should be used
for most cases for pressure,
when solving a natural convection problem
including gravity,
second order pressure
could lead to unphysical results,
and the pressure discretization
must be changed to either PRESTO! or Body-Force Weighted.
Going further down,
for Momentum, and other equations
such as Turbulent Kinetic Energy,
Specific Dissipation rate and
Energy equation in our case,
there are four different discretization methods
that are available in Ansys Fluent,
which can be seen by clicking on
any of the drop-down menus here.
The second order upwind is set by default
for obtaining the most accurate solution
on a suitably refined numerical mesh.
The only reason that I would use the first order scheme
would be when a case is not converging to steady.
In this case I would first make sure that
mesh quality is acceptable,
and all my boundary conditions and physics
are correct and consistent.
After doing this
I would start the solution over,
doing some 50-100 iterations
using first order scheme
and then continue the solution with the second
order upwind.
Even for a ballpark estimate
I would move to first order
only in case of convergence issues.
For higher order estimates,
QUICK and MUSCL schemes can be used.
For a detailed discussion on the accuracy
of these methods,
please refer to the
Ansys Fluent Theory guide.
Other settings such as Warped-Face Gradient Correction,
High Order Term Relaxation
are available to be used if and when required.
These are advanced options
and are beyond the scope of this lesson.
Please refer to the User and Theory guides
to better understand the use-case for these options.
To summarize, in this lesson, we discussed
about the important parameters in the solution group
of the Solution tab
for the pressure-based steady-state solver.
We discussed about the pressure velocity coupling scheme
and learned about the different methods that can be used,
which are broadly classified into
segregated and coupled approaches.
We learned that for steady flow analysis,
the most robust scheme
is coupled with pseudo time method turned on
and set to Global Time Step.
Finally, we have also talked about the different
interpolation schemes
for other convection terms such as
energy, momentum etc.
With this
we have come to the end of our video.