Hello and Welcome!
In CFD, post processing is a term which describes all the ways
to interact with and examine the simulation results.
Post processing is done from the Results Tab in Ansys Fluent and it is typically
the last step in the CFD workflow.
In this demo lesson we will present a brief overview of using the Results Tab
of Ansys Fluent for both qualitative and quantitative
post processing using the heat sink geometry.
Sounds interesting, right? Let’s get started!
Before we get into our simulation,
let us get a clear idea of the problem being solved.
Here we have a geometry of a generic 3D heat sink with 5 fins made up of Aluminum.
The base of the heat sink is maintained at a constant temperature of 300K.
The model is assumed to be symmetric.
Air at 290K enters the domain with a velocity of 3m/s through the inlet.
The boundary conditions used are as shown here.
The goal of the simulation is to calculate the heat transfer
through the fins of the heat sink using 3D steady state simulation.
Let us now launch Ansys Fluent in Solution mode.
Go to File>Read, select Mesh and pick the mesh file.
After the mesh file is loaded, using the usual way of performing simulation using the Ribbon from left to right manner,
I will first go into the Domain Tab and perform the mesh check.
As you can see, there are no error messages displayed in the Console
and we can now proceed to the next Tab which is the Physics tab.
In the Solver group, I will set the Temperature in Reference values to 290 K.
Rest I will keep the defaults, which is usual practice for most cases.
In the Models group, I need to tick “Energy” so that Ansys Fluent will solve the energy equation
and calculate the temperatures.
I can see that Viscous is in blue, indicating that a turbulence model is active,
which is the default setting.
Because this is a turbulent flow,
no changes are required in the Models tab,
as the default Viscous model is the SST k-w turbulence model,
which is appropriate for our purpose.
Next, we will move to the materials group.
Since air is our working fluid and the fin material is Aluminum,
we do not have to make any modifications in the Materials group and Cell Zones tab,
as Air and Aluminum are the default materials in Ansys Fluent for fluid and solid zones respectively.
Let us now move ahead and click Boundaries.
I prefer to group them in zone type view, as it is more convenient to navigate through.
First, I will left click on inlet, ensure that it's the velocity-inlet boundary,
and click on edit. I want the inlet velocity to be 3 m/s.
In the thermal section, I will put the temperature at 290 K.
Then for sym-air and sym-solid,
I will use the symmetry boundary condition.
Moving to the outlet, it should be the pressure-outlet boundary with a 0 Pa gauge pressure.
Let’s see the wall boundaries.
When we speak of the base wall of the heat sink in this case,
we need it as a heat source, so I will go to Edit
and enter the value of temperature as 300 K.
I will leave all other walls at the default no-slip boundary condition.
Now that we have successfully defined materials, Cell Zones, and Boundary conditions;
we will now move to the next Tab, which is the Solution Tab.
Here, the default settings in the Methods and Controls groups
are appropriate for our need and we do not have to make any changes.
We will now move to the Reports group.
I want to define two report definitions for monitoring convergence.
I'll start by defining a force report.
When the panel opens, I'm going to choose Drag and enter a meaningful name.
Now, I will switch to Drag force from Drag coefficient and choose wall-sink-air from zones.
When writing force reports, it's important to choose the right force vector.
I'll modify the direction here to positive z,
since Drag force is in line with the main flow direction,
which is along the z-direction.
I'll check the Report Plot and Report File checkbox before clicking OK.
For the next report definition, I will go to Surface report
and then choose mass weighted average.
I will name this as outlet-temp-report,
the variable will be temperature and the surface will be outlet.
Rest of the settings are the same as the previous report definition.
Now I will initialize the solution using hybrid initialization.
Before running the simulation, I will save the initial case and data files.
Go to File>>Write>>Case & Data and save the file.
In the Run calculation group, Set the number of iterations to 200
and click on Calculate to initiate the solution calculation.
You can see that the solution is complete and converged.
Now, I will move to the next tab, i.e., the Results tab,
which is all about post-processing the results.
While post-processing, I would like to check first mass and energy balances,
to further ensure a satisfactory convergence of the problem,
which can be done through the fluxes option located under the reports group.
I will begin with the mass flow rate.
For that I will select the inlet and the outlet boundaries,
then click Compute.
The signs shown here convey the direction of mass flow;
the mass entering the domain is represented by positive sign and vice versa.
The sum of these values must be as close to zero as possible to satisfy conservation of mass.
In net results you can see that the sum, which is in fact a negligibly small value,
represents a good mass balance in the numerical simulation.
To check the energy balance, I will change the report to Total heat transfer
and select inlet, outlet and the walls
which are involved in the heat transfer.
Now, after computing it, you can observe the net result to be negligible again.
This means that we have a good energy balance in our case.
Both these checks provide additional confidence
on the convergence of our simulation.
Let us now conduct some quantitative post-processing to understand the solution results.
I will start by using the Surface Integrals panel.
This panel has many different report types
and is similar in function to the panel for surface report definitions.
The pressure drop is a significant quantity of interest in many CFD solutions,
so if I return to the previous panel and choose area weighted average with static pressure as the variable,
I may click the input and output under surfaces and compute.
Here, the figure given in the panel is the average value across all chosen surfaces.
However, what is frequently fascinating and helpful is that if you go to the console window,
you can see that, it also shows the values for each individual surface.
If you want to know the difference in pressure between an inlet and an outlet,
you can often just select the inlet in the panel and,
as long as you're using the default zero pressure at the outlet,
the result will be the pressure drop.
Since the pressure drop is simply the inlet pressure less the outlet pressure,
you can take advantage of the fact that this is typically the case.
Now I will create two line surfaces for plotting solution data.
Go to Create>Line/Rake
and create lines for these endpoints.
I will enter these manually and create two lines,
Line 1 and Line 2 respectively as shown.
Next, I will create a mesh display object.
For this one, I just want to include the walls
and I will just click Save/Display.
You'll notice when I did that the object appears in the tree,
and as you keep working, all the objects you create will be accessible from the tree.
Now to display the lines with mesh, Right click on mesh graphics,
which we have created previously in Outline View
and click Display.
Now drag the line-1 and line-2 from surfaces in Outline View
to the Graphics window.
This will help in visualising the lines in a better manner.
Moving on to the Plots Group, there is an option referred to as the XY Plot.
Here, I want to create a temperature graph along the line 2 that we have created above
to examine how temperature fluctuates across the model.
In order to do this, I'll click XY Plot > New
and choose line-2 from Surfaces.
Choose the Y axis function for temperature and the X axis function for the direction vector.
I'll enter values for Plot Direction as [0, 0, 1] for the temperature fluctuation in the Z direction
along a line and click Save/Plot.
This displays the plot of temperature variation over the line.
At the point where the line contacts the heat sink,
there is a quick rise in temperature.
Additionally, a steady increase in temperature can be detected
when the line is in touch with the heat sink.
Furthermore, as soon as the contact with the heat sink is gone,
you can see the Temperature falling down
due to heat dissipation in air as a result of convection.
Now I will move onto the flow visualization or qualitative post-processing.
I will start by creating another mesh display object
that includes only the walls of the computational model.
I will just click Save/Display to display the mesh object.
Let’s analyze the Velocity and the Temperature
gradients qualitatively with the help of Contours.
To start with, I will create the contours on a plane passing through the heat sink.
For this I will first need to create a plane, using the create plane option in the Surface group.
It will be a YZ plane. You can see how I am able to drag the plane in it’s normal direction
by dragging this arrow.
I will drag it until it comes in the heat sink region.
Now as we have the plane at desired location, I will name it as YZ-plane and click create.
Now, in Contours -> New,
select that plane and create a contour for velocity
by selecting the velocity in Contours of dropdown menu
and click Save/Display.
Look in graphics window and you will see how the velocity contours look like.
Follow the same procedure for Temperature contour.
For this, I will select Temperature from Contours of dropdown menu
and Static Temperature from sub-menu.
This will display a contour of Temperature.
In this contour you can see how the heat dissipates due to the forced convection.
Let’s move to another option, which is Pathlines.
This option helps in visualising the paths of fluid flow
by setting a surface as a starting point.
I will create a new Pathlines graphics, which I would like to be released from line 1.
Also, I would like them to be colored by Static Temperature,
so I will select Temperature from ‘Color by’ dropdown menu.
Click on Save/Display and you can now see the Pathlines emerging from line-1 surface.
In Pathlines window we also have Pulse option for an animated visualisation of the pathlines.
I will select Continuous mode in Pulse Mode and click on Pulse,
so you can see how the animation looks like.
To stop the animation, click on ‘Stop!’.
We will save this Pathlines graphics as pathlines-1.
Similarly, we can create pathlines-2 emerging from the inlet surface by selecting
Inlet as our release surface and you can see how it looks.
Another option is the Vectors,
which is used to visualise the vector quantities on the selected surfaces.
For now, let’s create a vector graphics on YZ-plane. Click on Vectors>New.
I will create Vectors of Velocity and color them by Velocity Magnitude.
I will select YZ-plane from Surfaces and click on Save/Display.
Here in Vectors window, we have options for choosing Style of vectors and also,
we can scale them according to our convenience.
Let’s try scaling them by factor 2.
See how the size of arrows increases in Graphics Window.
There is another interesting option provided by Ansys Fluent
here in Outline View which is Scene.
Here we can create a scene of multiple existing graphics as per our convenience.
Right click on Scene and select New and Scene window will open.
You can observe here that various Graphics Objects are presented in the window
in checklist format so that you can select whatever you want.
For now, I will select Temperature Contour, Vector, Mesh, and Pathlines
that we have created previously.
We can also adjust the Transparency of Objects using the slider here.
Let’s make our mesh 50% transparent.
Name the scene as scene-1
and click on ‘Save& Display’.
Now you can see in Graphics Window how I created the Scene,
which I wanted with a transparent mesh.
Now I would like to save the solution data and all the post processing that we have done,
and for that I will go to File > Write and select Case & Data to save the case and data files.
That brings us to the end of this tutorial.
Let’s summarize what we learnt in this tutorial.
We began with a quick description of the problem that we are using in this tutorial,
which is the air flow over a heat sink geometry.
Then we quickly performed the setup and computed the solution for this problem.
After that we discussed how to post process the results of the simulation using Results Tab.
In that we first discussed about the Reports group and after creating required line surfaces,
we created XY plot to plot the temperature distribution along the line
passing through the fluid domain and the heat sink.
We then learnt how to create plane surfaces and plot contours, vectors and pathlines
using graphics group.
We also learnt how to overlay multiple graphics objects to create a scene.
With that, let’s wrap up the lesson.