Unable to render {include} The included page could not be found.

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.

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.

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.

In the Line Display tab, use the default setting:

You will see Centerline Temperature created under Report in the Outline tab.

Notes to Cornell MAE 4272 Students:

You need to repeat the FLUENT simulation with inputs from YOUR MEASUREMENTS in the lab. To compare the FLUENT results with experiment, you can export the FLUENT result into Excel. A sample comparison is shown below. The experiment data can be downloaded here.

You can export the data by clicking on the Export button in "Details of centerline temperature"

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.

Again in this case, the x-axis is the x-position along the pipe and the y-axis denotes temperature.

Notes to Cornell MAE 4272 Students:

You need to repeat the FLUENT simulation with inputs from YOUR MEASUREMENTS in the lab. A sample comparison is shown below. The experimental data can be downloaded here.

You can export the data by clicking on the Export button, as shown in the previous step.

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.

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.

Notes to Cornell MAE 4272 Students:

You need to repeat the FLUENT simulation with inputs from YOUR MEASUREMENTS in the lab. The experiment data can be downloaded here. A sample comparison is shown below.

You can export the data by clicking on the Export button, as shown in the previous steps.

Axial Velocity Profile before and after Heated Section

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).

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.

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.