{include: FLUENT Google Analytics}
h1. FLUENT - Turbulent Pipe Flow - Step 6
{panel}
[Problem Specification|FLUENT - Turbulent Pipe Flow - Problem Specification]
[1. Pre-Analysis & Start-Up|FLUENT - Turbulent Pipe Flow - Step 1]
[2. Geometry|FLUENT - Turbulent Pipe Flow - Step 2]
[3. Mesh|FLUENT - Turbulent Pipe Flow - Step 3]
[4. Setup (Physics)|FLUENT - Turbulent Pipe Flow - Step 4 *New]
[5. Solution|FLUENT - Turbulent Pipe Flow - Step 5 *New]
{color:#cc0000}{*}6. Results{*}{color}
[7. Verification & Validation|FLUENT - Turbulent Pipe Flow - Step 7 CFD Post]
[Problem 1|FLUENT - Turbulent Pipe Flow - Problem 1]
{panel}
{info:title=Useful Information}
[Click here|SIMULATION:FLUENT - Turbulent Pipe Flow - Step 6] for the FLUENT 6.3.26 version.
[Click here|SIMULATION:FLUENT - Turbulent Pipe Flow - Results FLUENT] for the FLUENT 12 version.
{info}
h2. Step 6: Results
After the solution is complete, close the FLUENT window to return to the Workbench window. Double click {color:#660099}{*}{_}Results{_}{*}{color} in the main Workbench window to open CFD Post, where we will be viewing the results. For a basic orientation on how to use CFD Post, pl. see the videos in the [results step of the Laminar Pipe Flow tutorial|SIMULATION:FLUENT - Laminar Pipe Flow - Results].
The following instructions show only how to view results using the "chart" option. But one should really start by viewing velocity vectors, velocity/pressure/TKE contours etc. and check that the solution looks basically right. The [Laminar Pipe Flow tutorial|SIMULATION:FLUENT - Laminar Pipe Flow - Results] walks you through the steps to view vectors and contours in CFD Post.
h4. Locations
Before viewing the results, we need to define the locations in CFD Post where we would like to view the results, namely the wall, centerline, and outlet.
*Insert > Location > Line*
Rename this location "Pipe Wall". Avoid naming locations in CFD Post with identical names to those used in FLUENT, this can cause problems. We will define the line by two points. Enter (0,0.1,0) for {color:#660099}{*}{_}Point 1{_}{*}{color} and (8,0.1,0) for {color:#660099}{*}{_}Point 2{_}{*}{color}. Change {color:#660099}{*}{_}Samples{_}{*}{color} to 100.
Repeat the process for the two other locations needed:
{table}
|Name|Point 1|Point 2|
|"Pipe Centerline"|(0,0,0)|(8,0,0)|
|"Pipe Outlet"|(8,0,0)|(8,0.1,0)|
h4. y\+
Turbulent flows are significantly affected by the presence of walls. The _k-epsilon_ turbulence model is primarily valid away from walls and special treatment is required to make it valid near walls. The near-wall model is sensitive to the grid resolution which is assessed in the wall unit _y\+_(defined in section 10.9.1 of the FLUENT user manual). We'll gloss over the details for now and use the following rule of thumb: select the near-wall resolution such that _y\+ > 30{_} or _< 5_ for the wall-adjacent cell when using the {color:#660099}{*}{_}Enhanced Wall Treatment{_}{*}{color} option. Look at section 10.9, _Grid Considerations for Turbulent Flow Simulations_, for details.
Let's plot _y\+_ values for wall-adjacent cells to check how it compares with the recommendation mentioned above.
*Insert > Chart*
Let's rename the graph "Wall Y plus". Also, change {color:#660099}{*}{_}Title{_}{*}{color} to "Wall Y plus".
*Data Series Tab*
Rename the data series to "Y plus". Next, change {color:#660099}{*}{_}Location{_}{*}{color} to Pipe Wall.
\\
\\ [!cfdpost1.png|width=350!|^cfdpost1.png]\\
\\
*X Axis Tab*
Change {color:#660099}{*}{_}Variable{_}{*}{color} to {color:#660099}{*}{_}X{_}{*}{color}.
*Y Axis Tab*
Change {color:#660099}{*}{_}Variable{_}{*}{color} to {color:#660099}{*}{_}Yplus{_}{*}{color}.
Click {color:#660099}{*}{_}Apply{_}{*}{color} and our chart should appear.
!Y plus Results.PNG|width=450!
As we can see, the wall \_y+_value is between roughly 1.35 and 2.45. Since this is less than 5, the near-wall grid resolution is acceptable.
Export the data to a _.csv_ file ("comma separated values") by clicking on {color:#660099}{*}{_}Export{_}{*}{color}. This file can be opened in Excel.
\\
\\ [!cfdpost2.png|width=350!|^cfdpost2.png]\\
\\
h4. Centerline Velocity
Next, we would like to make a graph of the axial velocity along the centerline. We will do this by creating another chart.
*Insert > Chart*
Rename this chart "Centerline Velocity", and change the title of the chart as well.
*Data Series*
Change {color:#660099}{*}{_}Name{_}{*}{color} to "Centerline Velocity", and this time set {color:#660099}{*}{_}Location{_}{*}{color} to "Pipe Centerline".
*X Axis*
Once again, change {color:#660099}{*}{_}Variable{_}{*}{color} to {color:#660099}{*}{_}X{_}{*}{color}.
*Y Axis*
Change {color:#660099}{*}{_}Variable{_}{*}{color} to {color:#660099}{*}{_}Velocity u{_}{*}{color}, which corresponds to the Axial Velocity.
Click {color:#660099}{*}{_}Apply{_}{*}{color} and our chart should appear.
!Centerline Velocity Results.PNG|width=450!
h4. Coefficient of Skin Friction
The definition of the skin friction coefficient was discussed in the [laminar pipe flow tutorial|SIMULATION:FLUENT - Laminar Pipe Flow].
Once again, insert another chart, naming and titling it Coefficient of Skin Friction. Rename the data series and choose Pipe Wall for Location. Plot X on the X Axis and the Skin Friction Coefficient on the Y Axis. When complete, your chart should match the image below:
!Updated Skin Friction Results.PNG|width=450!
We can see that the fully-developed value is _0.0085_. Compare this with what you'd expect from the Moody chart.
h4. Velocity Profile
We'll plot the axial velocity at the outlet as a function of the distance from the center of the pipe.
Insert another chart, naming and titling it "Outlet Velocity". Change the name of the data series, and set the Location to Pipe Outlet. This time, put Velocity u on the X Axis and Y on the Y Axis. When complete, your chart should appear as below:
!Outlet Velocity.PNG|width=450!
The axial velocity is maximum at the centerline and zero at the wall to satisfy the no-slip boundary condition for viscous flow. Compare qualitatively the near-wall velocity gradient normal to the wall with the [laminar case|SIMULATION:FLUENT - Laminar Pipe Flow Step 6]. Which is larger? From this, what can you say about the relative strengths of near-wall mixing in the laminar and turbulent cases?
Go to [Step 7: Verification & Validation|FLUENT - Turbulent Pipe Flow - Step 7 CFD Post]
[See and rate the complete Learning Module|FLUENT - Turbulent Pipe Flow]
Go to [all FLUENT Learning Modules|FLUENT Learning Modules] |