Page History

Step 6: Results

Velocity Vectors

One can plot vectors in the entire domain, or on selected surfaces. Let us plot the velocity vectors for the entire domain to see how the flow develops downstream of the inlet. First, click on Graphics & Animations . Next, double click on Vectors which is located under Graphics. Then, click on Display. Zoom into the region near the inlet. (Click here to review the zoom functionality discussion in step 4.) The length and color of the arrows represent the velocity magnitude. The vector display is more intelligible if one makes the arrows shorter as follows: Change Scale to 0.4 in the Vectors menu and click Display.

The laminar pipe flow was modeled asymmetrically; however, the plot can be reflected about the axial axis to get an expanded sectional view. In order to carry this out (Click) Display > Views... as shown below.


Higher Resolution Image
Under Mirror Planes, only the axis (or centerline) surface is listed since that is the only symmetry boundary in the present case. Select axis (or centerline)and click Apply, as shown below.



Then click Close to exit the Views menu. Your vector field should have been reflected across the axially axis as, shown below.


Higher Resolution Image
The velocity vectors provide a picture of how the flow develops downstream of the inlet. As the boundary layer grows, the flow near the wall is retarded by viscous friction. Note the sloping arrows in the near wall region close to the inlet. This indicates that the slowing of the flow in the near-wall region results in an injection of fluid into the region away from the wall to satisfy mass conservation. Thus, the velocity outside the boundary layer increases. By default, one vector is drawn at the center of each cell. This can be seen by turning on the grid in the vector plot: Select Draw Grid in the Vectors menu and then click Display in the Grid Display as well as the Vectors menus. Velocity vectors are the default, but you can also plot other vector quantities. See section 27.1.3 of the user manual for more details about the vector plot functionality.

Centerline Velocity

Here, we'll plot the variation of the axial velocity along the centerline. In order to start the process (Click) Results > Plots > XY Plot... > Set Up.. as shown below.


Higher Resolution Image
In the Solution XY Plot menu make sure that Position on X Axis is selected , and X is set to 1 and Y is set to 0. This tells FLUENT to plot the x-coordinate value on the abscissa of the graph. Next, select Velocity... for the first box underneath Y Axis Function and select Axial Velocity for the second box. Please note that X Axis Function and Y Axis Function describe the x and y axes of the graph, which should not be confused with the x and y directions of the pipe. Finally, select centerline under Surfaces since we are plotting the axial velocity along the centerline. This finishes setting up the plotting parameters. Your Solution XY Plot should look exactly the same as the following image.


Higher Resolution Image
Now, click Plot. The plot of the axial velocity as a function of distance along the centerline now appears.


Higher Resolution Image
In the graph that comes up, we can see that the velocity reaches a constant value beyond a certain distance from the inlet. This is the fully-developed flow region. At this point the graph will be modified such that the fully developed regions results are truncated. That is, the range of the axes will be reconfigured. Open the Solution XY Plot menu, then click on Axes..., as shown below.


Higher Resolution Image
Then, deselect Auto Range, which is located under Options. The boxes under Range should now be accessible. Next, select X, which is located under Axis. Enter 1 for Minimum and 3 for Maximum under Range. At this point the grid lines will be turned on in order to help estimate where the flow becomes fully developed. Check the boxes next to Major Rules and Minor Rules under Options. At this point your Axes - Solution XY Plot menu should look exactly the same as the image below.


Higher Resolution Image
Lastly, click Apply. Now, that the X axis has been formatted, we will move on to formatting the Y axis. Select Y under Axis and once again deselect Auto Range under Options. Then, enter 1.8 for Minimum and 2.0 for Maximum under Range. Also select Major Rules and Minor Rules to turn on the grid lines in the direction. At this point your
Axes - Solution XY Plot menu should look exactly the same as the image below.


Higher Resolution Image
We have now finished specifying the range for each axis, so click Apply and then Close. At this point, the graph can be replotted. Go to the Solution XY Plot menu and click Plot to plot the graph again with the new axes extents.


Higher Resolution Image
From the image above, one can see that the fully-developed region starts at around x=3m and the centerline velocity in this region is 1.93 m/s.

Saving the Plot

In this section, we will save the data from the plot and a picture of the plot. The data from the plot will be saved first. In order to save the plot data open the Solution XY Plot menu and then select Write to File, which is located under Options. The Plot button should have changed to Write.... Click on Write..., and then enter vel.xy as the XY File Name. Next, click OK. Check that this file has been created in your FLUENT working directory. Lastly, close the Solution XY Plot menu.

...

Verify that the image file has been created in your working directory. You can now copy this file onto a disk or print it out for your records.

Coefficient of Skin Friction

FLUENT provides a large amount of useful information in the online help that comes with the software. Let's probe the online help for information on calculating the coefficient of skin friction. In order to access the online help first (click) Help > Users Guide Index as shown in the following image.



Click on S in the links on top and scroll down to skin friction coefficient. Click on the first link (normally, you would have to go through each of the links until you find what you are looking for). There you can see the following excerpt on the skin friction coefficient as well as the equation for calculating it.



Click on the link for Reference Values panel, which tells us how to set the reference values used in calculating the skin coefficient. In order to set the reference values, click on Reference Values, as shown below.



Then, set Compute From to inlet, to tell FLUENT to calculate the reference values from the values at inlet. Check that density is 1 kg/m3 and velocity is 1 m/s. (Alternately, you could have just typed in the appropriate values). Your Reference Values should look the same as the following screen snapshot.


Higher Resolution Image
Now, reopen the Solution XY Plot menu. Uncheck the Write to File check box under Options, since we want to plot to the window. The Options and Plot Direction can be left as is since we are still plotting against the x distance along the pipe. Under the Y Axis Function, pick Wall Fluxes..., and then Skin Friction Coefficient in the box under that. Under Surfaces, only select pipe_wall. At this point, your Solution XY Plot menu should look exactly like the following image.


Higher Resolution Image
Now, the ranges of each axis will be specified. Click on Axes... within the Solution XY Plot menu and re-select Auto-Range for the Y axis. Click Apply. Set the range of the X axis from 1to 8 by selecting X under Axis, entering 1 under Minimum, and 8 under Maximum in the box (remember to deselect Range Auto-Range first if it is checked). Click Apply, then click Close. Lastly, click Plot in the Solution XY Plot menu. You should obtain the following plot.


Higher Resolution Image
We can see that the fully developed region is reached at around x=3.0m and the skin friction coefficient in this region is around 1.54.
In order to save the data from this plot, first reopen the Solution XY Plot menu. Then, select Write to File under Options and click Write.... Enter cf.xy for XY File and click OK.

Velocity Profile

In this section we will plot the velocity at the outlet as a function of the distance from the center of the pipe. In order to start the process (Click) Results > Plots > XY Plot... > Set Up.. as shown below.


Higher Resolution Image
For this graph, the y axis of the graph will have to be set to the y axis of the pipe (radial direction). To plot the position variable on the y axis of the graph, uncheck Position on X Axis under Options and choose Position on Y Axis instead. To make the position variable the radial distance from the centerline, under Plot Direction, change X to 0 and Y to 1. To plot the axial velocity on the x axis of the graph, select Velocity... for the first box underneath X Axis Function, and select Axial Velocity for the second box. Next, select outlet, which is located under Surfaces. Then, uncheck the Write to File check box under Options, so the graph will plot. Your Solution XY Plot, should look exactly like the image below.


Higher Resolution Image
Next, click on Axes in the Solution XY Plot menu. Then, change both the x and y axes to Auto-Range. (Don't forget to click apply before selecting a different axis). Click Close in the Axes - Solution XY Plot menu.
It is of interest to compare the velocity profile with the theoretical parabolic profile. In order to plot the theoretical results, first click here to download the necessary file. Save the file to your working directory. Next, go to the Solution XY Plot menu and click Load File... and select the file that you just downloaded, profile_fdev.xy. Lastly, click Plot in the Solution XY Plot menu. You should then obtain the following figure.


Higher Resolution Image
Notice, how results compare relatively well with the theoretical parabolic profile. In order to save the data from this plot, first reopen the Solution XY Plot menu. Then, select Write to File under Options and click Write.... Enter profile.xy for XY File and click OK.
To see how the velocity profile changes in the developing region, we will add profiles at x=0.6m (x/D=3) and x=0.12m (x/D=6) to the previous plot. In order to create the profiles, we must first create vertical lines using the Line/Rake tool. First, (Click) Surface < Line/Rake as shown in the following image.



We'll create a straight line from (x0,y0)=(0.6,0) to (x1,y1)=(0.6,0.1). Select Line Tool under Options. Enter x0=0.6, y0=0,x1=0.6, y1=0.1. Enter line1 under New Surface Name. Click Create.



To see the line that you just created,(Click) Display > Mesh. Note that line1appears in the list of surfaces. Select all surfaces except default-interior. Click Display. This displays all surfaces but not the mesh cells. Zoom into the region near the inlet to see the line created at x=0.6m. (Click here to review the zoom functionality discussion in step 4.) The white vertical line appearing to the right is line1, as shown in the image below.



Similarly, create a vertical line called line2at x=1.2; (x0,y0)=(1.2,0) to (x1,y1)=(1.2,0.1). Display it in the graphics window to check that it has been created correctly. Now, we can plot the velocity profiles at x=0.6m (x/D=3) and x=0.12m (x/D=6) along with the outlet profile. First, open the Solution XY Plot menu. Under Surfaces, in addition to outlet, select line1 and line2. Make sure Node Values is selected under Options. Now, your Solution XY Plot menu should look exactly like the following image.


Higher Resolution Image
Lastly, click Plot and you should obtain the following output. Your symbols might be different from the ones below. You can change the symbols and line styles under the Curves... button. Click on Help in the Curves menu if you have problems figuring out how to change these settings.


Higher Resolution Image
The profile three diameters downstream is fairly close to the fully-developed profile at the outlet. If you redo this plot using the fine grid results in the next step, you'll see that this is not actually the case. The coarse grid used here doesn't capture the boundary layer development properly and under predicts the development length.

In FLUENT, you can choose to display the computed cell-center values or values that have been interpolated to the nodes. By default, the Node Values option is turned on, and the interpolated values are displayed. Node-averaged data curves may be somewhat smoother than curves for cell values.

Go to Step 7: Verification & validation

See and rate the complete Learning Module

Go to all FLUENT Learning Modules