Hello and Welcome!
In this workshop we will demonstrate
how to use the Ansys Fluent Meshing Watertight Geometry Workflow
to generate a simulation-ready mesh
for studying the fluid flow through a catalytic converter.
While generating the volume mesh
we will see how to use the Region-based sizing method
to locally refine the mesh.
We will also see how to rename the zones
using Manage Zones task,
after generating the volume mesh.
With the intention to prevent the backflow while simulating,
we will see how to extend the outlet boundary
using an additional task in the workflow.
Finally, we will demonstrate how to switch to the solution mode,
not only using the GUI but also using a TUI command.
Without further delay, let’s get started!
Launch Ansys Fluent in meshing mode.
For this demonstration, double precision is enabled,
and 4 processes are engaged for meshing.
Once Fluent Meshing launches,
select Watertight Geometry workflow.
In the Import Geometry task,
leave all the settings to default and load the provided geometry file.
The model we have here is that of a Catalytic converter,
which is an exhaust emission control device and is usually used with the IC engines.
The geometry consists of a solid domain of the catalytic converter
and three fluid domains i.e.,
the inlet cone region,
the porous region, which is a catalyst,
and the outlet cone region.
Let’s start with the workflow.
We will not be adding any local sizing.
Next, in the ‘Generate the Surface Mesh’ task,
keep the minimum size to the default value
and set the maximum size to 4 mm,
which is approximately 10% of the inlet diameter.
To ensure the presence of an appropriate number of cells
in the thin geometrical features of the solid domain,
set the Cells Per Gap to 2.
Note that, the solid domain of the imported geometry
does not have labels or named selections
defined at the CAD level
and hence it is considered as a single entity,
as can be seen here.
Therefore, we will have to separate the zones based on angles
while generating the surface mesh.
This is necessary for extruding the solid boundary
along with the fluid boundary,
after generating the volume mesh.
Therefore, set this option to ‘yes’ and
keep the Separation Angle to its default value.
Leave rest of the inputs to their default settings
and click on Generate the Surface Mesh.
Once the surface mesh has been generated,
notice how we have 2 cells along the thickness of the solid body,
compared to 1, when cells per gap is set to 1.
In the ‘Describe Geometry’ task, select the 3rd option for the geometry type,
as the imported geometry contains both the solid and the fluid regions.
Keep the ‘Will you cap openings and extract fluid regions?’ option to No
and set ‘Change all fluid-fluid boundary types from ‘wall’ to internal’?’
option to Yes.
This will allow the fluid to flow across the different fluid regions.
As we have already performed share topology operation at the CAD level,
we will set this option to No.
Click on ‘Describe Geometry’ button to execute the task.
In the Update Boundaries task,
ensure that appropriate boundary type for the boundaries is set
and then move to the next task
i.e., Create Regions.
As we have three fluid regions, set the ‘Estimated number of Fluid Regions’ to 3
and click on Create Regions button.
Note that, fluent has detected only 2 fluid regions,
as can be seen here in the list
and as reported in the console window.
However, as we can manually update the name and the type of regions
in the update regions task,
set the region type to fluid for the porous_region.
Next, in the add boundary layers task,
add 3 layers on the walls of the fluid regions,
and 1 layer on the solid-fluid interface of the solid region,
keeping rest of the inputs to their default settings.
Adding boundary layer in the solid region will help to accurately predict
the temperature gradients while performing the CHT analysis.
Finally, we will move to the ‘Generate the Volume Mesh’ task.
In this case of catalytic converter, the flow is wall-bounded and directional.
It is physically sensible to use poly-hexcore mesh,
wherein the hex cells of the resulting mesh will be aligned with the flow direction.
Set the Fill with Method to ‘Poly-Hexcore’.
Also, set the ‘Merge back the separated boundary zones?’ option to no,
to facilitate the extension of the solid boundary along with the fluid boundary,
after generating the volume mesh.
Make sure that the ‘Mesh Solid Regions’ option is ticked
before executing the task.
Hit the Generate the Volume Mesh button to create the volume mesh.
Once the mesh is generated,
observe the cut section.
For accurate modelling of the porous media while simulating,
it is generally advised to refine the mesh in that region.
Hence, we will use Region-based sizing method
to locally refine the mesh in the porous region.
Click on revert and edit to make the modifications.
Now, change the Sizing Method from Global to Region-based.
As soon as the Sizing Method is set to Region-based,
a table will pop up in the properties section,
which is populated with the region names and the corresponding Max cell lengths.
Here, the user can change the Max cell length as needed.
To refine the mesh, set the max cell length to 3 mm for the porous region.
Note that, the solver automatically updates the max cell length value ,
closest to the user specified value,
that reflects the actual max size as per the octree meshing scheme.
Click on Update button to generate the volume mesh.
Once the mesh is generated, observe the cut section.
As expected, the mesh is now refined in the porous region.
The mesh has a total of approximately 0.34 M cells
with a mesh quality of 0.2,
which is well above the recommended value of 0.1.
It is always a good practice to maintain the zone names
according to the zone type.
If not named earlier, we can still do it after generating the volume mesh,
with the help of the ‘Manage Zones’ task in the workflow.
Right-click on the 'Generate the Volume Mesh' task,
select 'Insert new task' and
click on 'Manage Zones'.
Select the ‘in_region’ cell zone,
set the operation to rename and enter the new name.
Click on Manage Zones button to execute the operation.
Similarly, rename the ‘out_region’ and ‘porous_region’ cell zones.
The ‘face zones’ can also be renamed in a similar way,
but let’s skip that for brevity.
Now, we will extend the outlet boundary,
which can prevent possible backflow during simulation.
Add the ‘Extrude Volume Mesh’ task in the workflow.
Select outlet boundary for both solid and fluid domain
using the graphics window.
Set the total height to 100 mm
with the number of layers as 20
and the growth rate as 1.1.
Once the task is executed, notice how the surface mesh of the original outlet boundary
is swept in the normal direction to create an extension.
Once the mesh is simulation-ready, it can be transferred to the Ansys Fluent fluid flow solver.
Simply click on ‘Switch to Solution’ button, located on top left corner of the ribbon
to transfer the mesh to Ansys Fluent solver.
Alternatively, user can also invoke the ‘switch-to-solution-mode' text command in the console window,
as shown here.
That brings us to the end of this workshop.