Hello and Welcome!
In this video, we will learn about the inputs that are required in the Add Boundary Layers task of
the Ansys Fluent Meshing Watertight Workflow.
The methods available for defining the boundary layer mesh depend on these inputs,
and hence it is critical to understand what each of these inputs mean.
Let’s get started.
We are well aware of the concept of boundary layers in fluid dynamics
and their influence on the overall fluid flow.
These thin, viscosity-dominant regions that form along the surface of the solid body as a fluid flows past it,
play a significant role in defining skin-friction drag, heat transfer, aircraft wing stall etc.
Hence, it is critical to ensure that CFD simulations properly model the physics of the fluid flow in these regions.
In addition to using appropriate numerical schemes,
it is necessary to ensure that the mesh in these regions is fine enough to adequately capture fluid flow behavior.
For this purpose, the watertight workflow in Ansys Fluent Meshing has a dedicated task
i.e., the ‘Add Boundary Layers’, which can be used to define the meshing requirement in the boundary layer zone.
Let us now take a look at how to use this task using an example.
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 Update Regions task have already been successfully completed.
This is because the surface mesh that we just imported into Fluent has originally been created using the watertight workflow
and saved after completing Update Regions task.
Such files when read back into Fluent retain the information regarding their workflow.
The model we have here is that of a generic ball or check valve,
which consists of 1 solid region i.e., the pipe geometry
and 3 fluid regions i.e., the inlet pipe region, the valve region, the outlet pipe region.
The ball valve is considered as a void in the model.
Let us now look at the ‘Add Boundary Layers' task.
If the ‘Add Boundary Layers’ setting is set to ‘yes’, multiple input options are populated below this setting.
The ‘Name’ field can be used to specify a name to the applied control settings.
By default, the name is auto-populated based on the Offset Method Type that is chosen.
The offset method controls how the first cell layer or the mesh cells closest to the solid boundary are generated.
There are 4 different offset method types,
i.e. smooth-transition, last-ratio, aspect-ratio and uniform.
Each of these methods have their own set of inputs to determine the height of the first cell layer.
Before we understand the methods, we need to first understand what the inputs are
and their role in boundary layer mesh generation.
The only input that is common to all the methods is the Number of Layers.
As the name suggests, it is the number of boundary layers that the user wants to create.
The default is 3.
Note that this number strongly depends on the accuracy requirement
needed for resolving the boundary layer flow.
For external aerodynamic flows such as flow over an aircraft or a car,
10-20 layers are commonly used to ensure the capture of all the necessary flow physics.
If the offset method is set to any method other than the last-ratio,
a growth rate input needs to be provided.
This is simply the ratio of the thickness of the next boundary layer cell to the previous boundary layer cell,
as viewed away from the surface on which the layers are being grown.
The default value is 1.2.
That means, if the first boundary layer thickness is x, the next layer’s thickness is 1.2 times x, and the one after that is 1.2^2 x,
and so on.
For scale resolving type simulations such as LES,
a lower value of 1.1 is generally used to make sure the chaotic aspects of the boundary layer fluid flow are sufficiently resolved.
If the offset method is set to smooth-transition or last-ratio,
a transition ratio value needs to be provided.
This value is the ratio between the height of mesh in the last boundary layer and the first cell in the volume fill.
A smaller value of transition ratio, closer to 0, implies a big jump in size between the boundary layer mesh and the volume mesh,
and on the other hand, a higher value, closer to 1,
implies that the cell height in the last boundary layer is comparable to that of the adjacent volume mesh cell.
When the offset method is set to last-ratio or uniform,
a first height value needs to be provided.
This value is nothing but the thickness of the first layer of the boundary layer mesh.
This value is very critical, especially in turbulent flows,
as most of the turbulent models require a certain specific first cell height to be used,
usually defined using a variable called the y+.
When the offset method is set to aspect-ratio, a first aspect-ratio value needs to be defined.
This is the ratio of the local surface mesh size to the height of the first cell in the boundary layer mesh.
Since the surface mesh is already created, the local mesh size is already known,
and the algorithm calculates the local first boundary layer thickness
using this local surface mesh size and the user entered aspect ratio.
Let’s summarize what we learnt in this lesson.
We briefly discussed the importance of boundary layers in fluid dynamics and
why it is critical to accurately capture the flow physics in these regions.
We then looked at the ‘Add Boundary Layers’ task, specifically the inputs that are required,
in the Ansys Fluent Meshing Watertight Geometry Workflow,
which can be used to define the boundary layer mesh.
With that let’s wrap up this video.