Hello and welcome to this video on the overview of the meshing process using Ansys Fluent
Meshing watertight workflow.
In this video, we will look at the bird’s eye view of the process of converting a CAD
model to a CFD simulation-ready mesh using the watertight workflow in Ansys Fluent.
We will learn how to launch a Fluent Meshing session, select the workflow, and go through
its different tasks to create a computational mesh that can be passed onto the fluid flow solver.
Along the way, we will also learn about a few items related to the workflow interface
such as tasks, task states, and more.
So, let’s get started!
Let’s start with launching a new session of Fluent meshing.
Start Fluent to open the launcher menu.
Here we can select Meshing to enter the meshing mode.
As you can see meshing is only available for three-dimensional geometries.
You can select whether to run in double precision, which is the recommended setting, and whether
to display the mesh after reading the file.
Over here you can input the number of processes to be used to enable parallel meshing and
accelerate the meshing process.
We will use 4 for our example.
Now, press start.
This is the Fluent Meshing interface.
In this video, we will focus only on the left side of the UI.
The drop-down menu in the workflow tab lets you choose between watertight geometry, fault-tolerant
meshing or creating a new workflow.
Select watertight geometry.
The buttons on the top-right of the panel let us load a saved workflow, save the current
workflow as a template, reset the entire workflow, or access the online help guide.
Let’s now briefly understand the various steps involved in creating a volume mesh using
Ansys Fluent Watertight workflow.
The meshing process can be broadly categorized into 4 major steps: importing the geometry,
setting mesh sizes and creating the surface mesh, describing the geometry and creating
regions (like solids or fluids), and finally setting up and generating the volume mesh.
Let’s go through this workflow with a simple example.
Click on the import geometry task to access its input panel.
Keep the default values for the file format and units and click on the three dots next
to the file name entry to locate and load the geometry file into the workflow.
For demoing the workflow, we will use a simple cylindrical pipe model.
Our aim is to create a volume mesh for this geometry, which can be used to simulate a
fluid flow through the cylindrical pipe.
Once the geometry is imported, you can notice that the import geometry task is now marked
by a green check mark.
This indicates that the task has been completed, while the yellow lightning with an exclamation
mark next to the remaining tasks indicates that these tasks have not been completed yet.
These icons are referred to as task states.
In addition to the green checkmark and the yellow lightning symbol there are 2 other
task states: A green check mark with an asterisk referring to a task that is completed but
with warnings for the user to review, and the red triangle with an exclamation mark
referring to a task that requires further attention.
The next task is to set up the local sizing settings for creating the surface mesh.
In this example, we will not be adding any local sizing, therefore, let’s leave the
choice to ‘No’ under add local sizing and press update.
In the input panel of the generate surface mesh task, change the minimum size to 1 millimeter.
Leave the rest at default and select generate the surface mesh.
Once the task is completed, a tessellated mesh representation of the cylindrical pipe,
generally referred to as a surface mesh, is created.
The next step is to describe the computational model which is done in the describe geometry task.
Because the geometry we imported represents the fluid flow region inside the cylindrical
pipe, we will select the option “the geometry consists of only fluid regions with no void”.
Leave the rest to default and press describe geometry.
In the next task i.e., update boundaries, we can specify the boundary conditions that
we would like to apply to the model.
The boundary surfaces have already been named during the CAD creation stage, which is the
recommended approach.
Based on these names, Fluent Meshing tries to automatically assign appropriate boundary conditions.
Like you see here, the wall surface has been assigned the wall boundary condition type.
Let us set Face1 to pressure-outlet and Face2 to velocity-inlet and press update boundaries.
Once a task is updated and is executed successfully without warnings or errors, all the tasks’
input options and controls are disabled.
If you need to make any changes to the inputs of a completed task, for e.g., say you wanted
to have the flow moving inside the tube in the opposite direction, so we need to flip
the boundary conditions applied on Face1 and Face2.
For this, you can use the ‘Revert and Edit’ button in that task’s input panel, perform
the necessary changes, in this case, assign velocity-inlet to Face1 and pressure-outlet
to Face2, and hit the update button to re-execute the task.
Notice how the tasks’ state changed from green checkmark to the yellow lightning symbol
indicating an incomplete task after hitting the ‘Revert and Edit’ button, and then
back to the green checkmark when the update button is selected.
Some tasks give you the option to ‘Edit’ instead of just ‘Revert and Edit’.
This is merely a cosmetic aspect to differentiate between tasks where user selection of zones
or labels was done, for which ‘Revert and Edit’ button is displayed, and those tasks
where only numerical inputs were provided, for which just ‘Edit’ button is displayed.
Note that you can edit any of the tasks in the workflow and not just the last performed
task.
However, all the tasks downstream of the task being modified will also have to be updated,
whether or not any changes were made to their settings.
Back to our workflow, in the next task which is the update regions task, simply press update
regions since we have only a fluid region.
Next, we need to choose whether we want to create boundary layer mesh for our model or
not.
In this example we won’t add any boundary layer treatment so select no under add boundary
layers and press the button below to move forward in the workflow.
In the last task, we need to provide inputs to generate the volume mesh.
Select fill with poly-hexcore, keep the other default values and press generate the volume
mesh.
In a matter of seconds, we obtain a high-quality mosaic-type mesh for our model.
That completes the meshing process, and you now have a volume mesh which you can pass
on to the Fluent solver to perform CFD simulations.
In addition to the tasks that are displayed by default in the workflow, you can access
additional tasks and task specific context menu by right-clicking on any of the tasks.
Here, not only do you get the flexibility to group, rename, or delete the selected task,
but also the option to insert and execute additional tasks.
Note that the contents of the ‘Insert Next Task’ option are dynamic and change through
the workflow based on which task you performed the right-click on.
For example, the task-specific context menu for the ‘Generate the volume Mesh’ task
gives you the option to add new tasks like extrude or transform the mesh, which are not
available anywhere else in the workflow.
Before we wrap-up this video, let’s quickly discuss about a few settings which can come
in handy, especially in situations where editing of completed tasks is needed to be done frequently.
These settings can be accessed by going to File -> Preferences and selecting Meshing
Workflow.
The ‘Save task editing data with mesh file’ option is turned on by default.
This option is to ensure that workflow-specific task editing data is saved when you save the
mesh file.
The data will be saved in a corresponding folder in the same location as where you saved
the mesh file.
When this option is enabled, the ‘Saving data for editing tasks’ will be automatically
set to ‘Write mesh files.’
This option instructs Fluent to save a mesh file whenever a completed mesh-related task
is edited and is the recommended selection to re-access the data in future sessions.
If this option is turned off, there are 3 options for ‘saving data for editing tasks’
setting.
In addition to ‘Write mesh files’, there is ‘write into memory’ which saves mesh
file information to the system memory while editing tasks, and ‘do not save data’
that does not save a mesh file when editing a task.
If ‘do not save data’ is selected and you need to edit a completed task, all the
upstream tasks up to the selected task will be re-processed.
This can be time taking, especially for large, complex models.
Other options here allow us to change the location of temporary files folder, or turn
on verbosity, which instructs fluent to print task-related messages to the console window.
The option ‘Task based display’ controls how Fluent displays task-specific items of
the model in the graphics window based on the threshold values set for ‘automatic
display face zone limit’ and ‘automatic display facet limit’.
This can be useful when displaying large models.
Lets summarize what we learnt.
We have seen how to start a Fluent Meshing session and select watertight meshing workflow.
We explored the overall look of the watertight workflow and its different tasks.
We discussed about different task states and their meaning, and also explored additional
settings to customize the workflow behavior.
That brings us to the end of this video.