Sign-up for free online course on ANSYS simulations!Useful Information
Click here for the FLUENT 12
Step 6: Analysis & Results
Centerline Velocity
We'll plot the variation of the axial velocity along the centerline.
Main Menu > Plot > XY Plot...
Make sure that Position on X Axis is set under Options, and X is set to 1 and Y to 0 under Plot Direction. This tells FLUENT to plot the x-coordinate value on the abscissa of the graph.
Under Y Axis Function, pick Velocity... and then in the box under that, pick Axial Velocity.
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.
Click Plot.
This brings up a plot of the axial velocity as a function of the distance along the centerline of the pipe.
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.
Change the axes extents: In the Solution XY Plot window, click on Axes.... Under Options, deselect Auto Range. The boxes under Range should now be activated. Select X under Axis. Enter 1 for Minimum and 3 for Maximum under Range.
We'll turn on the grid lines to help estimate where the flow becomes fully developed. Check the boxes next to Major Rules and Minor Rules under Options. Click Apply.
Now, pick 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. We have now finished specifying the range for each axes, so click Apply and then Close.
Go back to the Solution XY Plot menu and click Plot to replot the graph with the new axes extents. We 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
Save the data from this plot:
In the Solution XY Plot Window, check the Write to File box under Options. The Plot button should have changed to Write.... Click on Write.... Enter vel.xy as the XY File Name and click OK. Check that this file has been created in your FLUENT working directory.
Now, save a picture of the plot:
Leave the Solution XY Plot Window and the Graphics Window open and in the main FLUENT window click on:
File > Hardcopy ...
Under Format, choose one of the following three options:
EPS - if you have a postscript viewer, this is the best choice. EPS allows you to save the file in vector mode, which will offer the best viewable image quality. After selecting EPS, choose Vector from under File Type.
TIFF - this will offer a high resolution image of your graph. However, the image file generated will be rather large, so this is not recommended if you do not have a lot of room on your storage device.
JPG - this is small in size and viewable from all browsers. However, the quality of the image is not particularly good.
After selecting your desired image format and associated options, click on Save...
Enter vel.eps, vel.tif, or vel.jpg depending on your format choice and click OK.
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.
Main Menu > Help > User's Guide Index...
Click on S in the links on top and scroll down to skin friction coefficient. Click on the second link (normally, you would have to go through each of the links until you find what you are looking for). We can see an excerpt on the skin 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.
Set the reference values:
Main Menu > Report > Reference Values...
Select inlet under Compute From 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). Click OK.
Go back to the Solution XY Plot menu. Uncheck Write to File under Options since we want to plot to the window right now. We can leave the other Options and Plot Direction 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, select wall and unselect centerline by clicking on them.
Reset axes ranges: Go to Axes... and re-select Auto-Range for the Y axis. Click Apply. Set the range of the X axis from 1 to 8 by selecting X under Axis, entering 1 under Minimum, and 8 under Maximum in the box (remember to de-select RangeAuto-Range first if it is checked).
Click Apply, Close, and then Plot in the Solution XY Plot Window.
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. Compare the numerical value of 1.54 with the theoretical, fully-developed value of 0.16.
Save the data from this plot: Pick Write to File under Options and click Write.... Enter cf.xy for XY File and click OK.
Velocity Profile
We'll next plot the velocity at the outlet as a function of the distance from the center of the pipe. To do this, we have to set the y axis of the graph to be the y axis of the pipe (the 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, for X Axis Function, pick Velocity... and Axial Velocity under that.
Since we want to plot this at the outlet boundary, pick outlet under Surfaces.
Change both the x and y axes to Auto-Range. (Don't forget to click apply before selecting a different axis)
To compare the velocity profile with theoretical parabolic profile, click Load File... and select profile_fdev.xy
Uncheck Write to File under Options so that we can see the graph. Click Plot.
Does this compare well with the theoretical parabolic profile?
Save the data from this plot: Pick 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, let us add the profiles at x=0.6m (x/D=3) and x=0.12m (x/D=6) to the above plot. First, create a line at x=0.6m using the Line/Rake tool:
Main Menu > Surface > Line/Rake
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 just created, select
Main Menu > Display > Grid...
Note that line1 appears 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.) line1 is the white vertical line to the right in the figure below.
Similarly, create a vertical line called line2 at x=1.2; (x0,y0)=(1.2,0) to (x1,y1)=(1.2,0.1) in this case. 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. In the Solution XY plot menu, use the same settings as above. Under Surfaces, in addition to outlet, select line1 and line2. Make sure Node Values is selected under Options. Click Plot. 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.
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 underpredicts 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.
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.
Main Menu > Display > Vectors... > 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.
You can reflect the plot about the axis to get an expanded sectional view:
Main Menu > Display > Views...
Under Mirror Planes, only the axis surface is listed since that is the only symmetry boundary in the present case. Select axis and click Apply. Close the Views window.
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.
Go to Step 7: Refine Mesh