...

...

...

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 Image Removed. 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.
Image Removed

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.
Image Removed

...

Numerical Results

Temperature Contour

<iframe width="560" height="315" src="https://www.youtube.com/embed/7_P7arvK-4Q?rel=0" frameborder="0" allowfullscreen></iframe>

Summary of the Above Video:

1. Create a Contour Plot and name it Temperature Contours
2. Under Geometry > Locations, choose periodic 1 and set the variable of interest as Temperature.
3. Under View > Apply Scale, enter (1, 30, 1)
4. Default Transform
   1. Apply Reflection about ZX Plane

You can save the image to a file using the camera icon indicated in the image below or using the Snipping Tool in Windows (you can search for it under Start > Programs).

Image Added

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 Image Removed. 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.
Image Removed

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.
Image Removed

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.

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

Image Removed

Image Removed

...

https://confluence.cornell.edu/download/attachments/111221576/velocity%20vector.png

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. 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 (6.096,0,0)

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

Click Apply.

Image Removed

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 temperate 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".
Image Removed
Moving on, please select the Data Series tab. This tab will help us specify the source of the chart data. Create a new data series Image Removed.  Change the name from Series 1 to FLUENT. Under Data Source, specify Centerline as Location. Click Apply. This should result in a plot like:

\[insert the picture here\]

We would like to verify our simulation results, to do this we are comparing to experimental data. Experimental data is can be downloaded here. Download it to a directory of your choice. Now, click a new data series Image Removed. Name it "Experiment". Under Data Source, select File and browse for the downloaded experimental data.

Image Removed

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.
Image Removed

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

Image Removed

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 have are now displaying experimental data using data points denoted by red diamonds.
Image Removed

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

Image Removed

...

https://confluence.cornell.edu/download/attachments/111221576/Centerline%20Temperature.png

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 very close to the 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 is the number of sample points used when plotting data)

Click Apply.
Image Removed

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

...

<iframe width="560" height="315" src="https://www.youtube.com/embed/HX27T78mQfg?rel=0" frameborder="0" allowfullscreen></iframe>

Summary of the Above Video:

1. Click Vectors > Name Velocity Vectors
2. In Details plot Velocity 
3. In Variable > Color by Variable
   1. Color by temperature
      
      

We see that the flow speeds up as the density decreases in order to keep the same mass flow rate.  

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

Wall Temperature Plot

<iframe width="560" height="315" src="https://www.youtube.com/embed/-Cvn7HPp9eY?rel=0" frameborder="0" allowfullscreen></iframe>

Summary of the Above Video:

1. Create location > Line
   1. Point 1: (0,.0294,0) Point 2: (6.045,.0294,0)
2. Create Chart
3. Under Data Series  > Location Select line you just created
4. X Tab 
   1. Plot X location
5. Y Tab
   1. Plot Temperature

The wall temperature values can be exported to a csv file (suitable for Excel) using the Export button highlighted below.

Image Added

Importing Experimental Data and Chart Formatting

We can import experimental data from a csv file using the procedure shown below. The csv file should contain two columns, corresponding to the x-axis and y-axis values, respectively 

<iframe width="560" height="315" src="https://www.youtube.com/embed/oy3xJrmWNLo?rel=0" frameborder="0" allowfullscreen></iframe>

Summary of the Above Video:

1. In details of Chart > New Series > Import Data from file
   1. Find file and click okay
2. Change how experimental data looks in CFD Post
   1. In Line Display under Series 2 > No Line > Symbols > Ellipse
3. Chart Details > General
   1. Give Title
4. Chart Details > Chart Display
   1. Font Sizes
   2. Grid Sizes

Note that the centerline temperature and pressure variations can be plotted by duplicating this plot as mentioned in the video.

Mixed Mean Temperature at an Axial Location

From energy conservation, we can show that the mixed mean temperature is constant in the flow development and mixing sections and varies linearly in the heated section. This is shown schematically in the following figure from the MAE 4272 lab manual.

Image Added

The slope of Tm in the heated section can be obtained from the following equation which is derived from energy balance in the heated section:

Image Added

Using the above equation, calculate the mixed mean temperature Tm at x=2.67 m. Remember to add the inlet temperature, otherwise you will just end up with the temperature difference between the mixed mean temperature and the inlet temperature (where we assumed the flow was fully mixed). An alternate procedure to calculate Tm involves integrating the temperature profile. This procedure is covered in the Verification & Validation section in the video entitled Check Energy Conservation via Mixed Mean Temperature Variation. If energy is conserved in the FLUENT simulation, the values calculated using the two procedures should match.

Wall Temperature at an Axial Location

For calculating the Nusselt no. at an axial location, we need the wall temperature at that location. The wall temperature at an axial location can be calculated in two ways:

• By interpolating the Tw vs. x values exported to Excel from the wall temperature plot obtained above. 
• By directly extracting the wall temperature at the desired location using the Probe function in the post-processor. 

The following video shows you the procedure for extracting the wall temperature at x=2.67 m using the Probe function; this value can then be used to calculate the Nusselt number. To repeat the calculation at a different axial location, you can right-click on appropriate items in the tree, duplicate and modify as necessary. You need to double-click on an item in the tree to modify it; this is easy to overlook.

<iframe width="640" height="360" src="//www.youtube.com/embed/mv3uDy7ZuCY?rel=0" frameborder="0" allowfullscreen></iframe>

Summary of the above video:

1. Create a line at x = 2.67
2. Go to Expressions, right click and click New
   1. Name Tw267
3. Right click in Definition box > Functions > CFD-Post > maxVal
4. Right click within the parenthese of maxVal > Variables > Temperature
5. Right click after the @ sign > Locations > x267
   

Nusselt No.

Cornell MAE 4272 students, Fall 2020: Please use the following procedure for calculating the Nusselt number at two axial locations in the heated section where the flow is thermally fully-developed.  

The convective heat transfer coefficient, h can be determined from Newton's law of cooling:

Image Added

The wall heat flux on the left hand side is known from the boundary condition. We have shown you how to get the wall temperature T_w at an axial location. Calculate the mixed mean temperature at the same axial location by evaluating the following integral using the procedure shown in the video in the Verification and Validation section. The title of the video is Check Energy Conservation via Mixed Mean Temperature Variation. 

Image Added

Once you determine h, you can non-dimensionalize it to get the Nusselt number.

The Nusselt number in the thermally fully-developed region should be the same at different axial locations. Why? Do your Nu values at the two axial locations compare reasonably well? Why or why not?

<iframe width="640" height="360" src="//www.youtube.com/embed/WiK1uBTdK-M?rel=0" frameborder="0" allowfullscreen></iframe>

<iframe width="640" height="360" src="//www.youtube.com/embed/NbdGrJTesZg?rel=0" frameborder="0" allowfullscreen></iframe>

<iframe width="640" height="360" src="//www.youtube.com/embed/6RNykoM86xA?rel=0" frameborder="0" allowfullscreen></iframe>

<iframe width="640" height="360" src="//www.youtube.com/embed/Jcht7CAPzAc?rel=0" frameborder="0" allowfullscreen></iframe>

<iframe width="560" height="315" src="https://www.youtube.com/embed/x-flaXXU7xg?rel=0" frameborder="0" allowfullscreen></iframe>

Input Summary

In older versions of FLUENT, you can view the input summary (model, material properties, boundary conditions, etc) by clicking on Report in the menu bar of FLUENT. A small window will pop up and you can print the selected input summary directly in FLUENT.

Image Added

Go to Step 7: Verification & Validation

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

...

https://confluence.cornell.edu/download/attachments/111221576/Wall%20Temperature.png

Although 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.

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".
Image Removed
Now click on Data Series tap to specify the location of the chart data. Create a new data series Image Removed.  Change the name 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.

Image Removed

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 Image Removed. Name it Experiment. Under Data Source, select File and browse for the downloaded experimental data.
Image Removed

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.

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

Image Removed

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

...

https://confluence.cornell.edu/download/attachments/111221576/centerline%20pressure.png

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 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.
Image Removed
 

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

...

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.
Image Removed

...

https://confluence.cornell.edu/download/attachments/111221576/Axial%20Velocity%20Profile.png

...

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.

Image Removed
 
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".

Image Removed
 
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.

Image Removed
 
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.

Image Removed

...

https://confluence.cornell.edu/download/attachments/111221576/Axial%20Velocity%20Profile%20after.png

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".
Image Removed
 
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.

Image Removed
 
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.
Image Removed

...

https://confluence.cornell.edu/download/attachments/111221576/Temperature%20Profile%202.png

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