Hello and Welcome!
In this lesson, we will discuss the importance of the volume mesh
and learn about the two different Fill With methods
for generating the Volume Mesh in the Ansys Fluent Meshing Watertight Workflow.
This lesson is part-1 of the
two-part series and will focus on
Tetrahedral and Polyhedra Fill With methods.
We will dig into finer details of these methods and
understand the user inputs required.
Let’s get started
Volume mesh generation is the process of discretizing or representing a
computational model using a large number of discrete volumes or cells,
within which the governing equations are solved.
Extreme care needs to be taken during this process
as the volume mesh has a significant influence not only on the
accuracy and convergence of the solution
but also on the total simulation time.
Therefore, to generate the volume mesh,
there is a dedicated task in
the Ansys Meshing Watertight Geometry Workflow,
i.e., the 'Generate the Volume Mesh',
which can be used to define specific meshing requirements.
Let us understand this task using a demo problem.
Launch Ansys Fluent in meshing mode.
Go to File, Read, and select Mesh,
and then pick the provided mesh file.
Once Fluent finishes reading the file,
you will notice that the watertight geometry workflow
has been automatically setup and all the tasks till
the Add Boundary Layers tasks
have already been setup.
This is because the surface mesh that we just imported into Fluent
has originally been created using
the watertight workflow and saved after completing
Add Boundary Layers task.
Such files when read back into Fluent
retain the information regarding their workflow.
The model we have here is that of a generic
two-element rear wing
found on a formula series type race car,
enclosed within a virtual wind tunnel.
Except for the inlet and the outlet,
all the other sides of the wind tunnel
and the wing geometry are considered as walls.
The model consists of only the fluid domain
with the wing considered as a void.
In the ‘Generate the Volume Mesh’ task,
the first option is the 'Fill with'.
This option determines the meshing method to be used for
generating the volume mesh in the computational model.
There are 4 different methods available, namely
polyhedra, tetrahedral, hex-core and poly-hexcore.
Basically, the name of these methods represents
the geometry or the shape of the cells to be used
while generating the volume mesh.
Based on the selection, a list of the basic and the advanced inputs is
populated below this option.
The hex-core and the poly-hexcore Fill With methods will be discussed in part - 2 of this lesson.
Let's look at tetrahedral and polyhedra Fill With methods now.
When the 'Fill with' option is set to tetrahedral,
the user is prompted with 'Growth Rate' and 'Max Cell Length' inputs.
Let’s understand each of them.
As the name suggests, the 'Growth Rate' is simply the
length-based size ratio of the next cell to the
previous cell as viewed away from the boundary or the boundary layer cap,
towards the interior of the domain.
By default, the value is 1.2
and the range is from 1 to 3.
Let's understand this with an example.
Here, when the growth rate is 1.1,
there is a slower increase in the cell size away from the boundary,
whereas for the growth rate of 3,
the increase in the cell size is substantial.
It is advisable to use smaller growth rate values to avoid artificial diffusion
and possible divergence of the numerical solution.
The next input is the 'Max Cell Length'.
This value is nothing but the maximum length of the cell in the volume mesh.
This value defines the size of the largest cell in the domain.
By default, Fluent automatically calculates this value
depending on the existing surface mesh of the
computational model.
However, the user can change the values as required.
Though a large cell size reduces the overall cell count
and with it the computational time,
it is critical to ensure that the max cell size used in the domain is
adequate to resolve the large-scale features of interest in the fluid flow.
Let us now look at the tetrahedral volume fill
approach in action.
Click on the ‘Generate the Volume Mesh’ button.
Once the volume mesh has been generated,
we can turn on the clipping plane and
visualize an x-cut of our geometry.
Notice that the volume is filled with tetrahedral cells,
and the prism layers are created along the wall surfaces
from the triangular surface mesh,
as can be seen here.
This mesh has approximately 2.5 million cells,
and the minimum orthogonal quality is 0.15.
The major advantage of tetrahedral mesh is its
flexibility and adaptability with complex geometries.
On the downside, for the wall-bounded flows,
it is difficult to align the mesh in the flow direction,
which may hamper the accuracy of the solution.
It is generally recommended to use prism layers
to avoid highly skewed tetrahedral cells at wall boundaries and
to reduce the overall high cell count.
In the polyhedral volume fill approach,
multiple tetrahedral cells are combined
to form a polyhedral cell
which reduces the overall cell count.
This mesh is widely used
because of the advantages over the other type of meshes.
So, let’s discuss polyhedra Fill With method in detail.
When the 'Fill with' option is set to polyhedra,
which is the default option,
the user is prompted with the same basic user inputs
as in the case of tetrahedral Fill With method.
With the default settings and the same surface mesh,
let’s generate the volume mesh for our demo problem.
Once the volume mesh has been generated,
we can turn on the clipping plane and
visualize an x-cut of our geometry.
In addition to the volume being filled with polyhedral cells,
notice that the triangular surface mesh has been
modified to create a polyhedral surface mesh
from which prism layers are grown into the
computational domain.
Each polyhedral cell is bounded by many faces (more than 7)
and is therefore surrounded by many adjacent neighboring cells,
hence resulting in better approximation of the gradients,
and lower numerical diffusion effects.
However, more neighbors means more memory storage
and hence a slightly higher computational cost,
which is generally offset by the overall decreased cell count.
The mesh has 0.56 million cells
which is about 1/5th of the tetrahedral mesh,
which is the major advantage of this method.
Note that this reduction in cell count is a result of combining
multiple tetrahedral cells to form
fewer polyhedral cells.
Care needs to be taken to ensure that
the final mesh is sufficient to capture all the required
fluid flow behavior.
The minimum orthogonal quality of the mesh is 0.21
which is also better than the tetrahedral mesh.
Let's summarize what we learnt in this lesson.
We discussed the importance of volume mesh generation in the CFD simulations
and how to use the 'Generate the Volume mesh' task
in the Ansys Fluent Meshing Watertight Geometry Workflow.
We specifically understood the details of the
along with their advantages and disadvantages.
With that, let's end this video.