FLUENT - Forced Convection - Step 6

Step 6: Results

Please make sure your project is saved in Workbench. Double click on Results in the Project Schematic window. This will open CFD-Post (the program used to analyze results from FLUENT computation.)

Overview

You may have noticed in previous sections, that the pipe looks extremely long and thin on the screen. In fact, due to the axisymmetric assumption, we have only modeled half of a 2D section through the pipe in our analysis. To be able to make full use of the results, we must:

1) Generate the results for the parameter investigated (e.g. temperature, pressure, velocity).

2) Mirror the result to reflect the result of the full pipe section.

3) Stretch the pipe in the radial direction to better view contours.

The  results shown below were obtained with a pipe length of 6.096 which is slightly different from the current length of 6.045. So your results might be slightly different from those shown below.

Temperature Contour

Our first challenge is the temperature contour. On the top menu, click on contour . We will be calling this contour "Temperature Contour", OK when done. On the left hand side, Details of Temperature Contour will allow you to select parameters relevant to the results we're looking for. In this example, the Locations is periodic 1, the Variable is Temperature. The number of contours is a personal preference, in this example, we have selected 100. This step tells CFD-Post we are looking to plot contours of temperature.

The next step is to mirror the image, this will make the results more intuitive and easier to understand. From the previous screen, select the View tab. This tab will allow us to adjust the appearance of the contour plot we have just generated. Check Apply Reflection/Mirroring. Select ZX Plane for Method. Choosing this option reflects the current model in the ZX plane and allows us to view the "full" pipe section.

Finally, we stretch the pipe in the radial direction. Select Apply Scale. Enter 30 for y-axis. This will stretch our model in the y (radial) direction by a factor of 30. Click Apply. 

After you click Apply, you will see that under Outline > User Locations and Plots, Temperature Contour is created. You will also see that the Temperature Contour is plotted in the Graphics window on the right. Under Outline > User Locations and Plots, uncheck Wireframe to see just the Temperature Contour in the Graphics window.

Higher Resolution Image

In developing the experiment, it was assumed that by the end of the adiabatic mixing stage, the flow will be well mixed. Do the results from the numerical solution simulation support this assumption?

Velocity Vectors

Our next challenge is to produce velocity vectors. This is a very similar process to creating the temperature contours above. On the top menu, click on vector . Name it "Velocity Vector" and click OK. Under Details of Velocity Vector, select periodic 1 for Locations. Select Velocity for Variable. This tells CFD-post we are looking for vector plots of velocity.

In the next step, we will specify the appearance of vector arrows. Select the Symbol tab. Enter 0.05 for Symbol Size. This again is dependent on personal preference.

Finally click Apply. You will see that under Outline > User Locations and Plots, Velocity Vector is created. Un-check Temperature Contour so that Graphics window shows just the Velocity Vector plot. You can mirror the plot about the axis as before. You can translate the model to look at flow development near the entrance. There is a toolbar option at top that puts you in translate mode. You can click on the z-axis to restore our original view.

Does the flow become fully developed at the end of the first section?

Centerline Temperature Plot

Now let's look at the temperature variation along the center-line of the pipe. To do this we need to first create a center-line:

Insert > Location > Line

Name it "Centerline" and click OK. On the lower left panel, you will see Details of Centerline. Enter the following coordinates.

Point 1 (0,0,0)

Point 2 (6.045,0,0)

Enter 50 for Samples. (This will be the number of sample points used when plotting data)

Click Apply.

You will see centerline created under User Locations and Plots.

In the experiment, we are only able to measure the temperature at two points. First, at the inlet of the pipe and second, after the adiabatic mixing stage. The simulation can show us the variation of temperature in between these two points.

To create the desired plot:

Insert > Chart 
Please name this chart "Centerline Temperature". You will see Details of Centerline Temperature appear on the lower left panel. Select the General tab and name the chart "Temperature Variation along Pipe Axis".

Moving on, please select the Data Series tab. This tab will help us specify the source of the chart data.  Change the name of the first data series from Series 1 to FLUENT. Under Data Source, specify Centerline as Location. Click Apply. On top of this would would also like to plot the experimental data, which can be downloaded here. Download it to a directory of your choice. Now, click a new data series . Name it "Experiment". Under Data Source, select File and browse for the downloaded experimental data.

Now that we have our data sources, we will proceed by specifying the axes. We want to see the variation of temperature with the length of the pipe. Therefore, temperature will be on the y axis of the chart and x-position on the x axis of the chart. We will start by defining the X-axis:

Click on X Axis tab. Next to Variable, choose X.

Now the y axis: Click on Y Axis tab. Next to Variable, choose Temperature.

Now that the chart specifications are defined, we want to customize the display. The default setting is to display all data series using line charts, but since we only have very few experimental points, it would be more logical to display the experimental data using data points: Click on Line Display tab.  Select "Experimental" . Next to Line Style, change Automatic to None. Next to Symbols, change None to Diamond. Change the color to red. Click Apply.We are now displaying experimental data using data points denoted by red diamonds.

You will see Centerline Temperature created under Report in the Outline tab.
This is what you should see in the Graphics window.

Higher Resolution Image

From this it is obvious the experimental data compares quite well to simulation results. This would be more accurate if we had more experimental data points to work with, but as it is not the case, we can only assume that the in between stages match just as well as the inlet and outlet temperatures.

Wall Temperature Plot

We will now investigate the temperature variation along the wall. To do this we need to create a new line on the simulation. It needs to be a horizontal line correponding to the wall.

Insert > Location > Line

Please name this line "Wall" . On the lower left panel, you will see Details of Wall. Enter the following coordinates.

Point 1 (0,0.0294,0)

Point 2 (6.045,0.0294,0)

Again 50 for the sample size

Click Apply.

You will see wall created under User Locations and Plots.

Next, we will repeat the previous process, but using this new line as source data. 
Insert > Chart

You will see Details of Wall Temperature appear on the lower left panel. Under General tab, please name the chart "Wall Temperature".

Now click on Data Series tab to specify the location of the chart data. Change the name of the first data series from Series 1 to FLUENT. Under Data Source, specify Wall as Location.

As before, we would also like to compare our simulation result with experimental data. Experimental data can be downloaded here. Now, click a new data series . Name it Experiment. Under Data Source, select File and browse for the downloaded experimental data.
!data series|width=350!

Again in this case, the x-axis is the x-position along the pipe and the y-axis denotes temperature.
 
As previously shown, we will specify how the chart should be displayed. The default setting is to display the data series in lines. Since we only have a few experimental points, we want them to be displayed in data points. Click on Line Display. Then click on experimental tab. Next to Line Style, change Automatic to None. Next to Symbols, change None to Diamond. Change the color to red. Click Apply.

This is what you should see in the Graphics window.

Higher Resolution Image

The experimental data are a fairly good match for what the simulation has predicted. The wall temperature in the experiment seems to be consistently higher than the simulation in the heated section. We will later check if refining the mesh improves this agreement.

Pressure Plot

Now let's us look at the pressure variation at the centerline. We can use the center-line we created earlier.

Next, we will create a chart using this Location data. 
Insert > Chart 
Enter "Axial Pressure" as Name. You will see Details of Axial Pressure appear on the lower left panel. Under General, name the chart "Pressure Variation along Pipe Axis".

Now click on Data Series tap to specify the location of the chart data. Change the name of the first data series from Series 1 to FLUENT. Under Data Source, specify Centerline as Location. The centerline was already created while doing the temperature variation along the center-line. If that chart was skipped please refer to that section on how to create a centerline.
We would also like to compare our simulation result with experimental data. Experimental data is can be downloaded here. Download it to the directory that you like. Now, click a new data series . Name it Experiment. Under Data Source, select File and browse for the downloaded experimental data.

Our purpose in this exercise is to study the pressure variation along the length of the pipe. Therefore our chart should show pressure in the y-axis and x-position in the x-axis.

In this case, our x-axis variable is x and our y-axis variable is pressure. 
We want to the chart to be displayed exactly the same way as for wall temperature and centerline temperature plots.

This is what you should see in the Graphics window.

Higher Resolution Image

The simulation results follow the experimental data quite closely, the general trend is that pressure decreases (almost linearly) as we move from the inlet towards the outlet of the pipe.

Axial Velocity Profile

Now, let's investigate the velocity profile at different lengths along the pipe. We are especially interested in the flow development before it enters the heated section. Then please divert your attention to the difference heat addition has on flow development.

Axial Velocity Profile before Heated Section

The heated section is from x-positions of 1.83m to 4.27m. To allow us insight into flow development before the heated section, we will begin by creating 4 lines of x-position less than 1.83m.

Insert > Location > Line

The first line will be to define the inlet. Accordingly, please name this line "Inlet" and click OK. On the lower left panel, you will see Details of Inlet. Enter the following coordinates. The coordinates are entered in terms of (x,y,z).

Point 1 (0,0,0)

Point 2 (0,0.0294,0)

We want to create a vertical line, parallel to the y axis, so check to make sure that the x and z coordinates are the same for both points.

Enter 50 for Samples.

Click Apply.
Please repeat the process for Preheat 1 (x = 0.6) Preheat 2 (x=1.2) and 3 (x=1.8)

To double check, the coordinates for the 4 lines should be:

Check that you have the following under Outline.

Now that we have enough intervals to understand the flow development before the heating. We should create a chart of the velocity profile at these lines.

Insert > Chart 
Enter "First Section Axial Velocity Profile" as Name. Again, Details of First Section Axial Velocity Profile will appear and please name the chart "Axial Velocity Profile".

Select the Data Series tab to specify the location of the chart data. Change the name of the first data series to Inlet. Under Data Source, specify Inlet as Location. Continue adding Data Source until we added all Inlet, Preheat 1, Preheat 2, and Preheat 3. Name them according to the figure shown below.

Now we will specify the X Axis parameter. Click on X Axis tab. Next to Variable, choose Velocity u. Next we will specify the Y Axis parameter. Click on Y Axis tab. Next to Variable, choose Y. Click Apply. You will see First Section Axial Velocity Profile created under Report in the Outline tab.
 
This is what you should see in the Graphics window.

Higher Resolution Image

Notice preheat 2 and preheat 3 lines yield almost the same velocity profile. This tells us that after preheat 2, the flow his almost fully developed.

Axial Velocity Profile before and after Heated Section

To make things more interesting, let's now compare the velocity profiles before and after the heated section. To do this, we need to first create lines after heated section

Insert > Location > Line
Name it "Postheat 1" and click OK. On the lower left panel, you will see Details of Postheat 1. Enter the following coordinates.

Point 1 (4.27,0,0)

Point 2 (4.27,0.0294,0)

Enter 50 for Samples. (This will be the number of sample points used when plotting data) Click Apply.

Create Postheat 2.
Insert > Location > Line

Name it "Postheat 2" and click OK. On the lower left panel, you will see Details of Postheat 2. Enter the following coordinates.

Point 1 (5,0,0)

Point 2 (5,0.0294,0)

Enter 50 for Samples. Click Apply.

Continue the same step for creating line Outlet (x=6.045m).

Now we will have enough interval to look at the flow development before and after the heating.  Let's create a chart to investigate this.

Insert > Chart 
Enter "Second Section Axial Velocity Profile" as Name. You will see Details of Second Section Axial Velocity Profile appear on the lower left panel. Under General, give the chart Title as "Axial Velocity Profile".
 
Now click on Data Series tap to specify the location of the chart data. Under Data Source, specify Preheat 3 as Location for the first data series. Change the name to x=1.8m. Continue adding Data Source until we added all Preheat 3, Postheat 1, Postheat 2, and Outlet. Name them according to the figure shown below.

 
Now we will specify the X Axis parameter. Click on X Axis tab. Next to Variable, choose Velocity u. Next we will specify the Y Axis parameter. Click on Y Axis tab. Next to Variable, choose Y. Click Apply. You will see First Section Axial Velocity Profile created under Report in the Outline tab.
This is what you should see in the Graphics window.

Higher Resolution Image

What we notice when comparing fully developed flow before and after heated section is that the flow increases in velocity after the heated section. As air is heated, the density decreases. So the velocity has to increase to maintain the same mass flow rate.

Temperature Profile

Now let's us look at the temperature profile before and after the heating section.

Insert > Chart 
Enter "Temperature Profile" as Name.  Details of Temperature Profile appears on the lower left panel, so please name the chart "Temperature Profile".
 
Now click on Data Series tab to specify the location of the chart data.  Under Data Source, specify Preheat 3 as Location for the first data series. Change the name to x=1.8m. Similarly, add the locations: Preheat 3, Postheat 1, Postheat 2, and Outlet. Name them according to the figure shown below.

 
Now we will specify the X Axis parameter. Click on X Axis tab. Next to Variable, choose Temperature. Next we will specify the Y Axis parameter. Click on Y Axis tab. Next to Variable, choose Y. Click Apply. You will see Temperature Profile created under Report in the Outline tab.This is what you should see in the Graphics window.

Higher Resolution Image

The plot shows  temperature is nearly uniform at the outlet (end of mixing section).

Go to Step 7: Verification & Validation

See and rate the complete Learning Module

Go to all FLUENT Learning Modules