Numerical Results
Some of 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.
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.) Click on z axis in the triad (at the bottom right of the graphics window) to get the view along the z-axis.
Temperature Contour
On the top menu, click on 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.Click Apply.
. We will be calling this contour "Temperature Contour",In order to see the temperature contours better, we stretch the domain in the radial direction by a factor of 30 (the aspect ratio of the pipe will not be maintained in this view). From the previous screen, select the View tab. Select Apply Scale as shown in the image below. Enter 30 for y-axis (i.e. radial direction). Click Apply.
We can also mirror the image about the centerline which will give us a view of the temperature contours above and below the centerline. This view is more intuitive and easier to understand. In the View tab, check Apply Reflection/Mirroring. Select ZX Plane for Method. Click Apply.
In ANSYS version 14.5, only the pipe cross-section below the centerline is displayed after using the mirroring option in this menu. You can work around this by applying the mirroring condition in the "Default transform" setting. To do this select "Default Transform" in the left-hand menu by double-clicking on it. Uncheck "Instancing Info from Domain", check "Apply Reflection" and select to mirror about the ZX Plane.
After you click Apply, you should get a Temperature Contour plot in the graphics window similar to the one below (your temperature values may be slightly different). In our plot, we have turned off the (unstretched) wireframe by going to Outline > User Locations and Plots on the left and unchecking Wireframe.
You can save the image to a file using the camera icon highlighted below or using the Snipping Tool in Windows 7 (you can search for it under Start > Programs).
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 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.
. Name it "Velocity Vector" and clickIn 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.
The velocity vectors are shown below:
You can zoom in and out and move the contour using the tools right above the contour:
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:
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:
Axial Velocity Profiles
Let's look at the velocity profiles before and after the heated section. To do this, we need to first create lines at x=1.83 m ((start of heated section), x=4.27 m (end of heated section) and x=6.045 m (end of mixing section).
First, create the line at x=1.83 m.
Insert > Location > Line
Name it "x183" and click OK. Enter the following coordinates (0.0294 m is the pipe radius).
Point 1 (1.83, 0, 0)
Point 2 (1.83, 0.0294, 0)
Enter 100 for Samples. Click Apply.
Similarly create lines at x=4.27 m and x=6.045 m.
Insert > Chart
Name this chart "Axial Velocity Profiles".
Select the General tab and name the chart "Axial Velocity Profiles".
Select Data Series tab. Change the name of the first data series to x=1.83 m. Under Data Source, specify x183 as Location.
Add a new data series by clicking on the "New" icon as shown below and repeat the above steps but for x=4.27 m.
Add a third data series by clicking on the "New" icon and repeating the steps for x=6.045 m. You should then have three items in the Data Series tab.
Specify x-axis variable: Velocity u
Specify y-axis variable: Y
Complete the plot. Here's what we get.
We notice that the flow accelerates due to the heating. As air is heated, its density decreases. So the velocity has to increase to maintain the same mass flow rate.
Temperature Profiles
Similarly, one can look at the temperature profiles before and after the heated section.
Duplicate the Axial Velocity Profiles chart by right-clicking on the plot name in the "tree" on the upper left. Rename it as "Temperature Profiles".
Double-click on "Temperature Profiles" in the tree view to edit its properties. This should be just below "Axial Velocity Profiles" in the list.
Change the title and x-axis variable (to Temperature). Click Apply. Here's what we get.
This plot shows that:
- the temperature increases in the heated section
- the temperature is much higher near the wall in the heated section
- the temperature is nearly uniform at the end of the mixing section
All these trends are as expected.
Mixed Mean Temperature
The following video shows you the procedure for calculating the mixed mean temperature at x=2.67 m. To repeat the calculation at a different axial location, you can right-click on appropriate items in the tree, duplicate and modify as necessary.
Nusselt No.
The following video shows you the procedure for calculating the Nusselt no. at x=2.67 m. To repeat the calculation at a different axial location, you can right-click on appropriate items in the tree, duplicate and modify as necessary.
Fanning Friction Factor
The Fanning friction factor, also called the skin friction coefficient, can be plotted using the procedure outlined in numerical results section of the laminar pipe flow tutorial (scroll down to the end). The reference values for density and velocity to be used need to be calculated using the procedure outlined in section 1.43 of the HT2 lab manual posted on Blackboard.
Input Summary
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.