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 line corresponding to the center-line:

Insert > Location > Line

Name it "Centerline" and click OK. On the lower left panel, you will see Details of Centerline. Enter the start and end locations of the line and the sampling frequency. Click Apply.

You will see centerline created under User Locations and Plots.

Insert > Chart
Please name this chart "Centerline Temperature". You will see Details of Centerline Temperature appear on the lower left.

We'll go through the tabs in the menu to specify the plot that we want. Select the General tab and name the chart "Temperature Variation along Pipe Axis".

Select the Data Series tab. Change Name and Location.

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 axial position on the "x-axis" of the chart.

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

Click on Y Axis tab. Next to Variable, choose Temperature.

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

Note 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.

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

Wall Temperature Plot

We will now plot the temperature variation along the wall. First, create a line corresponding to the wall.

Insert > Location > Line

Name it "Wall" (with capital W; otherwise you'll get a conflict with a reserved name). On the lower left panel, you will see Details of Wall. Enter the start and end locations of the line and the sampling frequency. Click Apply.

You will see wall created under User Locations and Plots.

Insert > Chart

Name this chart "Wall Temperature". You will see Details of Wall Temperature appear on the lower left panel.

Select the General tab and name the chart "Wall Temperature".

Select Data Series tab. Change the name of the first data series to FLUENT. Under Data Source, specify Wall as Location.

As before, specify x-axis variable to be X (i.e. axial length along the pipe).

Specify y-axis variable to be Temperature. Click Apply. You should see the following plot.

Note to Cornell MAE 4272 Students:

You need to repeat the FLUENT simulation with inputs from YOUR MEASUREMENTS in the lab and compare the FLUENT results for the wall temperature with experiment. A sample comparison is shown below.

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

Pressure Plot

Create a plot of the pressure variation along the centerline of the pipe. Steps for this are similar to the plot of the centerline temperature that we did earlier.

There is no need to create a new line. We can use the "centerline" created earlier.

Insert > Chart

Follow steps from the Centerline Temperature plot above, making appropriate modifications. You should see the following plot.

Note to Cornell MAE 4272 Students:

You need to repeat the FLUENT simulation with inputs from YOUR MEASUREMENTS in the lab and compare the FLUENT results for the pressure with experiment. A sample comparison is shown below.

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.