Include Page |
---|
...
|
...
|
Include Page |
---|
...
|
...
|
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.
Numerical Results
Note |
---|
Cornell MAE 4272 Fall 2020: For the canvas quiz, you should use the FLUENT inputs from this tutorial. Later, you will need to repeat the FLUENT simulation with inputs from YOUR MEASUREMENTS in the lab and compare the FLUENT results with the experiment. |
Temperature Contour
HTML |
---|
<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:
- Create a Contour Plot and name it Temperature Contours
- Under Geometry > Locations, choose periodic 1 and set the variable of interest as Temperature.
- Under View > Apply Scale, enter (1, 30, 1)
- Default Transform
- 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).
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.
HTML |
---|
<iframe width="560" height="315" src="https://www.youtube.com/embed/HX27T78mQfg?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the Above Video:
- Click Vectors > Name Velocity Vectors
- In Details plot Velocity
- In Variable > Color by Variable
- Color by temperature
- 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?
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.
Info | ||
---|---|---|
| ||
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.
Info | ||
---|---|---|
| ||
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.
Info | ||
---|---|---|
| ||
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.
The plot shows temperature is nearly uniform at the outlet (end of mixing section).
Go to Step 7: Verification & Validation
Wall Temperature Plot
HTML |
---|
<iframe width="560" height="315" src="https://www.youtube.com/embed/-Cvn7HPp9eY?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the Above Video:
- Create location > Line
- Point 1: (0,.0294,0) Point 2: (6.045,.0294,0)
- Create Chart
- Under Data Series > Location Select line you just created
- X Tab
- Plot X location
- Y Tab
- Plot Temperature
The wall temperature values can be exported to a csv file (suitable for Excel) using the Export button highlighted below.
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
HTML |
---|
<iframe width="560" height="315" src="https://www.youtube.com/embed/oy3xJrmWNLo?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the Above Video:
- In details of Chart > New Series > Import Data from file
- Find file and click okay
- Change how experimental data looks in CFD Post
- In Line Display under Series 2 > No Line > Symbols > Ellipse
- Chart Details > General
- Give Title
- Chart Details > Chart Display
- Font Sizes
- 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.
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:
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.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/mv3uDy7ZuCY?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the above video:
- Create a line at x = 2.67
- Go to Expressions, right click and click New
- Name Tw267
- Right click in Definition box > Functions > CFD-Post > maxVal
- Right click within the parenthese of maxVal > Variables > Temperature
- 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:
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.
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?
Wall Shear
We plot the wall shear using the procedure shown in the video below.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/WiK1uBTdK-M?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the above video:
- Click on the Chart Viewer tab
- Click chart in the top toolbar
- Name it Wall Shear
- Click on Data Series Tab
- In Location dropdown menu, choose Wall
- Click on X Axis tab
- under Variable, choose X
- Click on Y Axis tab
- under Variable, choose Wall Shear X or Wall Shear
- Go to Location in the tree
- Double click on Wall
- Increase Sampling from 50 to 200
We then consider the trends in the wall shear in the heated, mixing and flow development sections and try to justify them through physical reasoning.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/NbdGrJTesZg?rel=0" frameborder="0" allowfullscreen></iframe> |
You can spiff up your plot using the tips discussed below. This video also shows you how you could read in experimental results for comparing the wall shear between simulation and experiment.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/6RNykoM86xA?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the above video:
- To edit how the Wall shear graph is displayed
- Select Wall shear in tree
- Click on General, check Title and enter title in Title blank
- in Data Series, enter series name in Name blank
- in X Axis, enter x axis label in Custom Label blank
- same for Y Axis
- in Line Display, uncheck "Use series..." and type within Legend Name blank
- in Chart Display, under Sizes, toggle with the line sizes and font
- To add another data series
- go to Data series tab of Wall Shear
- click on New button
- Scroll down, click File as Data Source > browse for your file
- To export the chart
- Click the button next to undo
- Select location to save
- Rename
When the simulation was repeated for conditions for which experimental data are available, we got the comparison shown below. The difference in the average wall shear in the heated section between the simulation and experiment is a respectable 4%. Note that the wall shear in turbulent flows is difficult to predict accurately due to the steep velocity gradients at the wall.
Fanning Friction Factor
The Fanning friction factor, also called the skin friction coefficient, is obtained by non-dimensionalizing the wall shear. It can be calculated and plotted using the procedure outlined below.
HTML |
---|
<iframe width="640" height="360" src="//www.youtube.com/embed/Jcht7CAPzAc?rel=0" frameborder="0" allowfullscreen></iframe> |
Summary of the above video:
- Create Location > Point
- (2.67, .0294, 0)
- Probe wall shear at point:
- Create Expression > Right Click > New Expression
- probe(Wall Shear)@w267 / 1.483 (Pa/K) /Tm267
- Can duplicate for different locations for a plot
Final Plots
HTML |
---|
<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.
Go to Step 7: Verification & ValidationSee and rate the complete Learning Module