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
that can be used to study the conjugate heat transfer characteristics of a generic turbine blade geometry.
Using this simplistic model,
we will identify a non-standard workflow
that can significantly improve the meshing process
for complex turbine blade geometries.
Along the way,
we will also learn how to setup curvature local size control
to accurately resolve the curvature of the cooling passages,
employ manual rotational periodic boundaries,
and setup boundary layer mesh in both fluid and solid regions
to facilitate an accurate prediction of temperature gradients while performing the CHT analysis.
Let’s get started!
Turbines used in gas turbine engines
in various applications such as power generation, propulsion etc,
are placed downstream of the combustion chamber.
As a result,
they encounter fluid that is at extremely high temperature.
In addition to using high-temperature resistant material,
cooling strategies such as passing bleed air from compressor
through the blades via cooling channels is quite common.
Realistic turbine blades are extremely complex
with strong curvatures and long, narrow, winding cooling ducts.
Good care needs to be taken
while meshing such geometries
in order to create appropriate meshes
which can be used to accurately model the conjugate heat transfer process.
Because of the complexity of the turbine blade geometry,
there may be issues
during the CAD creation phase
associated with fluid domain extraction,
share topology
etc. In this workshop, we will demonstrate an alternative approach
using a simple turbine blade geometry,
which is also extendable to complex models,
that leverages the fluid domain extract feature of the watertight geometry workflow.
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 geometry consists of only 1 region
i.e., the solid domain of blade connected to the hub.
The blade has 10 cooling channels
that extend all the way from the top of the blade to the bottom of the hub.
The blade is enclosed within surfaces
that make up the boundaries of the fluid domain.
Select ‘yes’ for ‘would you like to add local sizing’ option
in the Add Local Sizing task.
To ensure that the cooling passages are sufficiently resolved,
we will impose a curvature local sizing on them.
Change the Size control type to ‘curvature’.
Set local min size to 0.1 and max size to 1 mm.
Leave rest of the settings to default
and pick the ‘wall_cooling_passages’ label from the list,
and click on Add Local Sizing to execute the task.
In the generate the surface mesh task,
set the minimum size to 0.1 mm.
Leave rest of the settings to default
and execute the task.
Next, it is time to setup the periodic boundary conditions.
Right click on the generate the surface mesh task
to show the task-specific context menu
and pick ‘Setup Periodic Boundaries’
from the Insert next task menu.
To virtually account for the multiple blades in the rotor row,
we will set the sides of the model to use a rotational periodic boundary condition.
Note that, the solid and fluid surfaces from each side were grouped together
to create the ‘periodic_1’ and ‘periodic_2’ labels
during the CAD creation phase.
This circumvents the limitation of being able to create only 1 set of periodic boundaries
when using the watertight geometry workflow.
In this demo,
we will illustrate how to manually setup the periodic boundaries.
Set ‘Type’ to Rotational and Method to Manual.
From the CAD,
we know angle between the two periodic face is 8 deg.
Enter this value in the periodic angle input.
Furthermore, the center of rotation can also be got from CAD,
which is entered here.
The rotation axis is in the negative y direction,
so enter 0, -1, 0 for the x, y, and z rotation-axis direction inputs respectively.
For the manual method,
only 1 periodic face needs to be selected
and second face is autodetected based on the above inputs.
Select ‘periodic_1’ from the list and execute the task.
A successful execution of the task indicates that the periodic boundaries were correctly defined
and setup.
In the Describe Geometry task,
select ‘the geometry consists of both solid and fluid regions and/or voids’
as the Geometry Type
and leave the rest of the options to their default.
Note that, even though we don’t have a fluid domain
and need to extract it,
we already created the boundary surfaces of the fluid domain
during the CAD stage
so, the ‘will you cap openings and extract the fluid regions’ option can be left to ‘no’.
In the update boundaries task,
all the boundaries should have been correctly assigned to their appropriate boundary conditions
based on the labels.
Ensure that these are correct and move onto the Create Regions task.
Here, Fluent estimates 1 Fluid region based on the geometry,
which is the correct estimation.
Leave this value as is and execute the task.
Next, we will add boundary layers to all the walls in the fluid domain of our model.
Therefore, set ‘Add Boundary Layers?’ option to yes,
leave all the settings to default
and execute the task.
Because the intent is to use the mesh for conjugate heat transfer analysis of the turbine blade,
it is generally recommended to create 1 boundary layer
in the solid region at the solid-fluid boundaries to accurately predict the temperature gradients.
In the Add Boundary Layers task,
set the number of layers to 1,
Add in to Solid Regions and Grow on to Solid-Fluid Interface
and click Add Boundary Layers.
Now we are ready to create the volume mesh.
For this demo, we will use the poly-hexcore fill with approach
to fill the core of the fluid domain with hexahedral cells
and connect them with the poly-prism cells at the boundaries
using polyhedral cells.
Leave the Buffer and Peel Layer inputs to default and
ensure that min and max sizes are set to 0.1 mm and 3.2 mm respectively.
Also make sure that the ‘Mesh Solid Regions’ option is ticked
so that the solid domain is also meshed.
Click on ‘Generate the Volume Mesh’ to create the volume mesh.
Here is the generated volume mesh.
You can clearly see identical mesh between the two periodic boundaries,
and 3 layers of boundary layer mesh in the fluid region and 1 layer in the solid region
at the solid-fluid interface.
In channels that are wide enough,
hexahedral cells are created,
however, for the narrow channels, no hex cells are created.
To ensure hex cells are created even in the narrow regions,
the minimum size should be reduced.
With that, let’s wrap up this workshop.