FLUENT - Forced Convection - Step 6

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 symmetry condition of the experiment, we have only modeled half 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

3) Adjust the scaling of the resulting graphs so that the variation of the pipe in y direction is more pronounced.

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.

Finally, we want to view the variation of parameters along the y axis of the pipe. This means we will need to "stretch out" the plot. Select Apply Scale. Enter 30 for y-axis. This will stretch our model in the y direction. 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 Visit page in new 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 . Please 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. Uncheck Temperature Contour so that Graphics window shows just the Velocity Vector plot.

It would be beneficial to repeat the previous steps involved with mirroring and stretching the plot:

Higher Resolution Image Visit page in new window

Please focus on the first section of the pipe as it shows flow development. Can you see at which point the flow becomes fully developed?

Centerline Temperature Plot

Now let's look at the temperature variation along the center-line of the pipe.

Insert > Chart
Enter "Centerline Temperature" as Name. You will see Details of Centerline Temperature appear on the lower left panel. Under General, give the chart Title as "Temperature Variation along Pipe Axis".

Now click on Data Series tap to specify the location of the chart data. Create a new data series . Change the name from Series 1 to FLUENT. Under Data Source, specify Centerline as Location.

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 to the downloaded experimental data.

Now we will specify the X Axis parameter. Click on X Axis tab. Next to Variable, choose X.

Now we will specify the Y Axis parameter. Click on Y Axis tab. Next to Variable, choose Temperature.

Now we will specify how we want to the chart to display. The default setting is to display the data series in lines. Since we only have 3 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. 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 Visit page in new window

Does the simulation result compares well with the experimental data?

Pressure Plot

Now let's us look at the pressure variation at the centerline. First, we will create a line call centerline.

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 (6.096,0,0)

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.
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, give the chart Title as "Pressure Variation along Pipe Axis".

Now click on Data Series tap to specify the location of the chart data. Create a new data series . Change the name from Series 1 to FLUENT. Under Data Source, specify Centerline as Location.

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 to the downloaded experimental data.

Now we will specify the X Axis parameter. Click on X Axis tab. Next to Variable, choose X.

Now we will specify the Y Axis parameter. Click on Y Axis tab. Next to Variable, choose Pressure.

Now we will specify how we want to the chart to display. The default setting is to display the data series in lines. Since we only have 3 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. You will see Axial Pressure created under Report in the Outline tab.

This is what you should see in the Graphics window.

Higher Resolution Image Visit page in new window

Does the simulation result compares well with the experimental data?

Wall Temperature Plot

Now let's us look at the temperature variation along the wall. First, we will create a line call wall.

Insert > Location > Line

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

Point 1 (0,0.0294,0)

Point 2 (6.096,0.0294,0)

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

Click Apply.

You will see wall created under User Locations and Plots.
Next, we will create a chart using this Location data.
Insert > Chart
Enter "Wall Temperature" as Name. You will see Details of Wall Temperature appear on the lower left panel. Under General, give the chart Title as "Wall Temperature".

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

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 to the downloaded experimental data.

Now we will specify the X Axis parameter. Click on X Axis tab. Next to Variable, choose X.

Now we will specify the Y Axis parameter. Click on Y Axis tab. Next to Variable, choose Temperature.

Now we will specify how we want to the chart to display. The default setting is to display the data series in lines. Since we only have 3 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. You will see Axial Pressure created under Report in the Outline tab.

This is what you should see in the Graphics window.

Higher Resolution Image Visit page in new window

Does the simulation result compares well with the experimental data?

Axial Velocity Profile

Now let's us look at the axial velocity profile at various location in the pipe. We are interested in the flow development before the heated section and would like to observe how heat addition in the heated section will affect the flow development. To do this, let's start with investigation the flow before the heated section.

Axial Velocity Profile before Heated Section

The heated section is from 1.83m to 4.27m. Let's create 4 lines before 1.83m in the pipe.

Insert > Location > Line

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

Point 1 (0,0,0)

Point 2 (0,0.0294,0)

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

Click Apply.

Create Preheat 1.

Insert > Location > Line

Name it "Preheat 1" and click OK. On the lower left panel, you will see Details of Preheat 1. Enter the following coordinates.

Point 1 (0.6,0,0)

Point 2 (0.6,0.0294,0)

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

Click Apply.

Continue the same step for creating line Preheat 2 (x=1.2m), Preheat 3 (x=1.8m).

Check that you have the following under Outline.

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

Insert > Chart
Enter "First Section Axial Velocity Profile" as Name. You will see Details of First 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. Create a new data series . Under Data Source, specify Inlet as Location. Change the name to Inlet. 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 Visit page in new window

Axial Velocity Profile before and after Heated Section

Let's 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=6.096m)

Check that you have the following under Outline.

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. Create a new data series. Under Data Source, specify Preheat 3 as Location. 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 Visit page in new window

The flow is accelerated in the heated section.

Temperature Profile

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

Insert > Chart
Enter "Temperature Profile" as Name. You will see Details of Temperature Profile appears on the lower left panel. Under General, give the chart Title as "Temperature Profile".

Now click on Data Series tab to specify the location of the chart data. Create a new data series. Under Data Source, specify Preheat 3 as Location. 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.