Hello and Welcome!
Once a CFD simulation is setup and solved in Ansys Fluent,
the solution data needs to be post-processed in order
to extract meaningful results.
An important aspect to understand about post-processing in Ansys Fluent
is that post-processing operations such as
contours, pathlines etc, are performed on surfaces.
In this lesson, we will learn about the most commonly used Surfaces
and how to create them.
So, without further delay let’s get started!
Post-processing is a general term that includes
all the ways that we interact with and examine the simulation results.
Post-processing can be broadly classified into two categories, qualitative and quantitative.
Qualitative post-processing involves contours, vectors, pathlines, and much more,
which can be used to visualize what the flow looks like
and is primarily used to gain a visual insight into complex flow phenomenon.
Quantitative post-processing involves XY Plots, histograms, averaged reports, forces,fluxes, etc.
Which can be used to get numerical data
to identify trends, patterns, comparison with
analytical, experimental or other similar simulation results.
All the necessary post-processing tools in Ansys Fluent are grouped under the Results tab.
Let us now use an example case to familiarize ourselves with the layout of the Results tab,
and to understand the process of creating post-processing surfaces.
Launch Ansys Fluent in Solution mode.
Once the Ansys Fluent solver launches, load the provided case and data files.
The Results tab is located to the right of Solution Tab.
In this tab, there are groups for graphics and plots
where we find various flow visualization operations
and there is also a group for reports which has different panels that can be
used to extract quantitative information from the solution data.
As mentioned earlier, in Ansys Fluent all post-processing operations are performed on surfaces.
Ansys Fluent has options to create many kinds of surfaces using the options under the Surface group.
To create Surfaces, we can either go to the context menu under Create > Surfaces,
or we can go to the outline view, right click on Surfaces
and choose New.
Let us now understand how to create the commonly used surface types i.e.,
point surfaces, plane surfaces and iso-surfaces.
First let’s look at the Point Surface.
The Point Surface, sounds like a contradiction but it's really just a point.
Suppose we want to monitor flow field variable at a particular location as
done by probes in experiments,
we can do so by creating a point surface.
The most commonly used approach when we are creating points
is just to type the coordinates in the panel.
There are two other approaches;
Using the mouse probe and selecting any location in the domain
to specify the point.
In this approach, the point tool automatically snaps to the nearest Node or Cell Center,
depending on the option selected in the Snap on Probe Click group box.
The other approach is to interactively move the point tool to the location in
the domain where you want the point surface to be created.
You can move the point tool by left-clicking and holding any of the axes
to move the point in that direction,
or by clicking the ball in the middle of the point tool to move it freely.
Simply click Create to define the point surface.
Now let’s look at plane surfaces.
There may be cases when we want to visualize the solution on a 2D plane
to understand the flow-field of the problem.
For example, a velocity contour, to see the boundary layer formation near the object.
In such a case, a plane surface can be used.
Plane surfaces can be created through the plane surface panel dialog box.
There are a variety of intuitive methods to define a plane.
It can be aligned with any of the Cartesian axes or we can also define the ‘point and normal'
or define three points through which the plane passes.
Depending on the method we pick, a variety of different tools are available
to help us position the plane in the graphics display.
For any of the three Cartesian plane methods, there's a tool that's aligned with the axis
using which you can interactively create the plane in the computational domain.
You can even directly define the location of the plane
by entering the coordinate of the chosen Cartesian axis
or there's also a select with mouse option which you can use
to interactively select a point in the computational domain to locate the plane.
You have the option to create multiple planes at a prescribed spacing.
Just increase the number of surfaces to a value greater than one,
enter a spacing greater than 0 and the display will update.
In the three-point method, you can position the plane
by interactively moving the plane tool i.e.,
by manipulating the axis triad located in the middle of the plane.
You can rotate on an axis, move the plane within a single axis,
or "grab" the center of the axis and relocate the point and the entire plane
anywhere within the domain.
Alternatively, you can either enter the coordinates for each of the three points
or select using mouse probe.
When using the point and normal method, you can position the plane interactively,
similar to the three-point method.
Alternatively, for defining the point you can either enter the coordinates of the point
or select using mouse probe.
For defining the normal, you can directly specify the end point of the normal through iX, iY and iZ,
or you can choose Compute from View Plane to position the plane normal
to your view in the graphics display window
or choose Compute from Surface and select a surface to position the plane normal to it.
For our case, we will just go ahead and choose ZX plane to create the plane surface.
The third most common type of surfaces are iso-surfaces.
There may be instances when we want to display the cells of model that have certain constant value of the selected variable,
for that iso-surfaces can be used.
First, we will choose a variable under Surface of Constant. Let’s just use Temperature.
Do not make any selection from the From Surface list if you want the isosurfacing to be performed on the entire domain,
and similarly do not select a zone from the From Zones list to avoid restricting isosurfacing to a specific cell zone
and instead run through the entire domain.
Now, when we click on Compute, the minimum and maximum value
of chosen variable from simulation result is displayed here.
Then if we move the slider bar, a temporary display of the iso-surface will appear
that corresponds to the value in the panel and if we move this back and forth we can see how the surface updates according to the value.
There is also an option to create offset surfaces,
similar to the option in the Plane Surface panel.
Instead of relying on the slider bar, the more common scenario is that we know the exact value
we want and that can be entered directly in the panel.
Note that when we enter the value directly, the temporary surface display does not update.
Simply click create to define the iso-surface.
If the surface is not displayed,
go to the Outline View and drag the surface into the graphics window.
Apart from the commonly used surfaces discussed till now,
there are other types of surfaces that can be created.
For example, to display results on a boundary,
we can create new zone surface.
Line and Rake surfaces can be used when we want to plot solution data variation along a line.
To display data on a line, plane, circle, sphere or general quadric surface,
we can create Quadric Surface by entering the coefficients of the quadric function that defines it.
To clip the surface between iso values and have it span a specified subrange of a selected scalar quantity,
the iso-clip method can be used.
Other surface types such as partition, imprint, structural point etc. can also be created.
Please refer to the user guide a detailed understanding
on how to create and use them.
Note that, all the surfaces that we create are listed under outline view,
and to make changes to a surface after it has been created,
just right click and choose Edit.
So, for the plane, let’s say we want it at a very precise value
and change the name to something more descriptive,
it is easy to do that.
We can edit surfaces at any time, and as often as we need.
The last option we will talk about is Manage.
The manage option in Surface group lets you edit, rename, delete, group and ungroup surfaces
and obtain information about their components.
The Surfaces dialog box that pops-up when the manage button is clicked
displays both surfaces created by the user
and the automatically generated surfaces based on the boundaries of the model.
Grouping surfaces is useful if you want to perform postprocessing on a number of surfaces at a time.
For example, you may want to group several wall surfaces together
to generate a contour plot of temperature on all walls.
To postprocess results on each wall surface individually simply “ungroup” the surfaces.
Additionally, various topological information such as surface type, number of points,
0D, 1D and 2D facets on the surface, and surface id of the selected surfaces
can also be obtained from the Surfaces dialog box.
Note that, grouping, ungrouping, and deleting can also be done
from outline view after selecting appropriate surfaces.
Let’s summarize what we learnt in this lesson.
We understood the concept of post processing,
and the different types of post processing options possible in Ansys Fluent.
Next, we learnt in detail about how to create three most commonly used surfaces namely,
point surface, plane surface and iso-surface.
Then we briefly discussed about the other surfaces
that are available in the surface group of the results tab for post processing.
Finally, we learnt about the various options available under
the Manage option of Surface group,
With that let’s wrap up the lesson.