Hello and Welcome!
In this lesson, we are going to understand how the 'Update Boundaries' task, which is
a sub-task of Describe Geometry, can be used to review and update the properties of boundaries
in the Ansys Fluent Meshing Watertight Geometry Workflow.
We will begin with learning different ways to modify the name and type of the boundaries,
and then understand how to display the boundaries either based on their type or a custom set
of selections.
We will also briefly touch upon how to merge zones by inserting an additional task in the workflow.
Let's get started.
Though modifying the name and type of the boundaries can be done in the fluent solver
after importing the mesh, it is recommended to do that in the meshing phase using the
'Update Boundaries' task in Watertight Geometry Workflow.
In addition to defining the boundary properties at the meshing level, by defining these even
before generating the volume mesh, the user can add boundary layers to particular boundaries
of interest i.e., the 'wall' type boundaries using the 'Add Boundary Layer' task, later
in the workflow.
Now, let us understand the 'Update Boundaries' task with an example.
The geometry here is that of a "Centrifugal Separator" with 3 fluid regions i.e., inlet
pipe, cone, and outlet pipe.
Named selections have been assigned for 'Inlet' and 'outlet' surfaces, and the share topology
operation has already been performed.
Now, launch fluent meshing, and select ‘Watertight Geometry.’
Import the provided geometry and execute 'Add local sizing' and 'Generate surface mesh'
tasks by keeping their default settings.
In the next task i.e., the 'Describe Geometry' task, as the geometry consists of only fluid
regions, select the 'only fluid' option for the geometry type.
Notice that the 'Update Boundaries' task appear in the workflow.
The 'Update Boundaries' task also appears when the geometry type is set to 'both fluid
and solid', but not when it is set to 'only solid', which will be discussed later in this video.
Since the fluid flow should be continuous across the three regions, set ‘Change all
the fluid-fluid boundary type from ‘wall’ to ‘internal’’ setting to ‘yes’.
We do not have to perform share topology here as it has already been performed at the CAD level.
Click on 'update' to move to the 'Update Boundaries' task.
In the properties section of the 'Update Boundaries' task, based on the selection type i.e., Label
or Zone, a list of boundary names is populated in the table.
For this demo, we will use the ‘Zone’ selection type.
Turn on the 'List all Boundaries' option to make the internal boundaries visible in the table.
If any of the boundary properties are modified and the ‘Update Boundaries’ task hasn’t
been executed, toggling the 'List all boundaries' option will discard all the modifications
made in the table.
Therefore, it is recommended to first toggle the 'list all boundaries' option before making any modifications.
In the table, notice that the boundaries with the pattern 'inlet' and 'outlet' in their
label, are assigned with 'velocity-inlet' and 'pressure-outlet' boundary type respectively.
This is because Fluent automatically assigns the appropriate boundary conditions based
on the boundary name.
Here is the list of typical naming conventions and the associated boundary conditions that
are automatically applied by Ansys Fluent.
To change the name of the boundary, either double-click on the boundary name and enter
the new name, or right click on the boundary name, select 'set boundary name', click on
the blank space and enter the new name.
Similarly, to change the boundary type, click on the drop-down menu in the 'Boundary type'
column and select the type from the list or right click on the boundary name, select 'Set
Boundary Type' and choose the appropriate type for the boundary.
Click on ‘Update boundaries’ once done.
To modify any properties, go back to 'Update Boundaries' task, click on 'revert and edit'
and make the necessary changes in the table and then click on ‘Update’.
It is also possible to modify the boundary properties, any time later in the workflow,
by manually adding the task.
This avoids the need for editing the original 'update boundary' task and updating all the
subsequent tasks.
To do this, right click on any of primary tasks between generate surface mesh and generate
volume mesh, select 'Insert Next Task' and click on 'Update Boundaries', and make the
necessary changes.
The Update Boundaries task can also be used to display boundaries in multiple ways.
To display a custom selection of the boundary surfaces, choose the required boundaries using
the left mouse button while keeping the control button pressed, right click on any one of
the selected boundaries and click on 'Draw Selections'.
To display the boundaries based on the type, click on the draw boundaries option, and select
the type of boundaries to be displayed on the screen.
In cases where modifications are required, make sure to first modify and execute the
task before using the 'Draw boundaries' option.
This ensures that the boundaries are displayed based on the updated properties.
Now, let us discuss the case when geometry consists of only solid regions.
When ‘The geometry consists of only solid regions' option is selected in the Describe
Geometry task, the 'Update boundary' task is not added to the workflow.
This is because Fluent by default assigns a 'wall' type to all the solid boundaries.
If fluid regions need to be extracted for these geometries, the 'Enclose Fluid Regions'
task can be used for creating the fluid region boundaries and assigning the appropriate boundary
types.
Nevertheless, ‘Update Boundaries' task can be manually added in the workflow in case
modifications are required for the boundary properties.
Let’s now discuss a special case when the imported geometry consists of multiple boundary
zones, within a region (or a cell zone), which need to be merged.
This can be done in the ‘Add boundary type’ task using the 'merge zone' operation.
For example, in this imported geometry, the inlet is split into 2 zones.
In this case, when boundary conditions are applied in the fluent solver, two separate
boundary conditions would be required to be assigned.
Therefore, it is advised to merge these zones during the meshing phase itself.
To do this, right click on Describe Geometry task, or any other task in the workflow, select
'Insert Next Task' and click on 'Add boundary type'.
A new task appears in the workflow.
This task is identical to the ‘Update Boundaries’ task except for ‘merge zones’ operation.
Now, select the zones to be merged, set the name, and select the boundary type.
Set the ‘Merge the zones?’
option to ‘yes’ and hit 'Add boundary type'.
A new boundary is created, which appears below the 'Add boundary type' task in the workflow.
The green tick mark shows that the boundary is updated without any errors or warnings.
Let us quickly recap what we learnt in this lesson.
We understood how to update the properties of any defined boundaries.
We also saw how to display boundaries based on their type or a custom set of selection.
Finally, we learnt how to merge zones using the 'Add boundary type' task.
That brings us to the end of this lesson.