Hello and Welcome! In this workshop, we will generate a simulation-ready mesh for studying the fluid flow in a generic mixing tank geometry,
using the Ansys Fluent Meshing Watertight Geometry Workflow. During the workshop we will explore how to perform share topology and
region-based volume meshing using the workflow. Finally, we will demonstrate how to extrude boundary surfaces of the volume
mesh. Let’s get started! Mixing tanks are constant volume tanks containing inlet ports, outlet ports and stirrers
also known as agitators or impellers. The rotation of the impellers, thoroughly mix the contents of the mixing tank. The analysis of
fluid flow in the mixing tank is necessary to troubleshoot any mixing issues and design an effective mixing tank. In this workshop, the
generic mixing tank geometry consists of a cylindrical tank with a tangential inlet, an outlet at the bottom and 4 baffles on the wall. Two
impellers with four blades each, are mounted on a central shaft. We will be considering only the fluid flow region of the mixing tank as our
computational domain. The rotation of the impellers is modeled using the Multiple Reference Frame (MRF) model. The MRF
model is a steady-state approximation in which individual cell zones can be assigned different rotational and/or translational speeds.
Therefore, separate fluid zones are required around the rotating parts to differentiate the moving zones from the stationary zones. In the
sectional view, notice there are three cell zones. Two of them are around the rotating impellers and the third cell zone is the
remainder of fluid in the tank. It should be noted that in the MRF approach, the moving zone mesh does not move and remains fixed
for the computation. For further details on the MRF model, please refer to the User’s Guide. Let’s now look at how to mesh this model.
Launch Ansys Fluent in meshing mode. Once Fluent Meshing is launched, select Watertight Geometry workflow. In the Import Geometry
task, leave all the settings to default and load the provided geometry file. Next, retain the ‘Would you like to add local sizing?’ option to
‘No’ in the Add local sizing task. We will be specifying the mesh size controls in the ‘Generate the Surface Mesh’ task. In this task,
change the minimum and maximum size to 3mm and 30mm respectively. Change the cells per gap to 2 and set the proximity-based
refinement to faces to resolve the baffle and impeller walls accurately. Keeping the rest of the settings to default, click on ‘Generate the
Surface Mesh’. Once the surface mesh is generated, ‘Apply Share Topology’ task is inserted in the workflow. As the share topology
operation was not performed during the CAD creation stage, Fluent automatically includes the share topology task in the workflow. In the
‘Describe Geometry’ task, set the geometry type to ‘only fluid regions with no voids’. Change all fluid-fluid boundary types from ‘wall’
to ‘internal’ as the interfaces between the different cell zones are not physical interfaces and fluid should be allowed to flow across
them. The share topology option will be set to ‘Yes’. Executing the ‘Describe Geometry’ task, will take you to the ‘Apply Share Topology’ task.
While retaining the default value of ‘Max Gap Distance’, we will check the gaps identified for sharing using the ‘Mark Gaps’ button. It clearly
shows that only the interfaces between the moving zones and the adjacent zone are marked for sharing. The default share topology
method of Join-Intersect is suitable here, therefore the task can be executed with the default settings.
In the Update Boundaries task, the wall liquid level represents the free surface of the liquid inside the tank, and we will model it as a
symmetry boundary. All the other boundaries are correctly identified by Fluent. After the boundaries are updated, the three regions in
the model are correctly identified as fluid type in the ‘Update Regions’ task. There are no changes to be made in this task, so we will
execute it and move onto defining the boundary layers. We will use the default smooth-transition method to grow the boundary
layer mesh from all the walls in the fluid region. Leave the settings to the default and select ‘Add Boundary Layers’ button to execute the
task. Now we are ready to generate the volume mesh. In this demo, we will use the ‘poly-hexcore’ ‘Fill With’ method to fill the core of the
fluid volume with hexahedral cells, which are connected to boundary layer mesh through polyhedral cells. We will use the ‘Region-based’
sizing method to obtain fine mesh in the MRF regions. This method allows us to assign different cell sizing controls, such as, growth
rate and the maximum cell size, to each available region. When poly-hexcore ‘Fill With’ method is selected only the ‘Max Cell Length’
needs to be specified for each region. Increase the number of buffer layers to 3 and set the ‘Max Cell Length’ to 6mm for both the
MRF regions. Keep the other settings to default and hit the Generate the Volume Mesh button to create the volume mesh. The generated
mesh has a total of approximately 1.1 million cells with a mesh quality of 0.2. The volume mesh can be inspected using the help of
‘Clipping Planes’. Notice the relatively fine mesh in the MRF regions and the boundary layers growing on tank and impeller walls. Fine
mesh in the MRF regions may also be obtained by applying body size type local size controls. In body sizing, the target mesh size sets the
size on both, the boundaries and the interior of the region. Setting the maximum cell length in region-based volume meshing, only controls
the size on the interior of the body and has no impact on the surface mesh like local sizing. If finer mesh is required at the impeller walls, the
recommended approach would be to provide a face size control with the desired target mesh size and provide an appropriate maximum cell
length in the MRF region during volume meshing. Next, we will demonstrate how to extrude
boundary surfaces using the ‘Transform Volume Mesh’ task. The mixing tank has an inlet and outlet port whose lengths we want to
increase. To do this, Right-click on ‘Generate the Volume Mesh’ task, go to ‘Insert New Task’ and select ‘Extrude Volume Mesh’. Retain the
method to ‘Total Height’ and select the ‘inlet’ and ‘outlet’ faces from the list. Enter 100mm for the ‘Total Height’, 10 for ‘Number of Layers’
and change the ‘Growth Rate’ to 1 to achieve uniform layer height. Click ‘Extrude Mesh’ button to execute the task. The inlet and outlet
faces have been extruded as per the specified inputs. Also notice that the location of the inlet and the outlet faces have shifted to a new
location due to the extrusion operation. The mesh is ready to be exported to the Fluent solver. Please note that, being a conformal
grid, this mesh can be used for only MRF simulations. While in the solver mode, if a need arises to simulate using the sliding mesh
approach, then some modifications will be required to be done in the solver to convert from MRF model to sliding mesh model. This
brings us to the end of the workshop.