Sign-up for free online course on ANSYS simulations!Step 6: Results
Velocity Vectors
One can plot vectors in the entire domain, or on selected surfaces. Here, the vectors will be plotted for the entire domain. First, click on Graphics & Animations . Next, double click on Vectors which is located under Graphics. Then, click on Display in the Vectors menu. You should obtain, the following output.
You can use the wheel button of the mouse to zoom into the region that closely surrounds the plate, to get a better view of the boundary layer velocities.
Outlet Velocity Profile
In this section we will first plot the variation of the x component of the velocity along the outlet. Then we will plot the Blasius solution to see how the numerical solution compares. In order to start the process (Click) Results > Plots > XY Plot... > Set Up.. as shown below.
In the Solution XY Plot menu make sure that Position on Y Axis is selected , and X is set to 0 and Y is set to 1. This tells FLUENT to plot the y-coordinate value on the ordinate of the graph. Next, select Velocity... for the first box underneath X Axis Function and select X 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 geometry. Finally, select outlet under Surfaces since we are plotting the x component of the velocity along the outlet. This finishes setting up the plotting parameters. Your Solution XY Plot menu should look exactly the same as the following image.
Now, click Plot. The plot of the x component of the velocity as a function of distance along the outlet now appears.
In order to increase the legibility of the graph, we will plot the data as a line rather than points. To turn on the line feature, click on Curves... in the Solution XY Plot menu. Then, set Pattern to ----, set the Weight to 2 and select nothing for Symbol, as shown below.
Next, click Apply in the Curves - Solution XY Plot menu. Next, close the Curves - Solution XY Plot menu.
Now, the range of the y axis will be truncated, as we are not interested in far field velocity. Furthermore, the grid lines will be turned on. In order to implement these two changes. First click Axes in the Solution XY Plot menu. Next, select Y for Axis, deselect Auto Range, select Major Rules, select Minor Rules. Then, set Minimum to 0 and set Maximum to 0.12. Your Axes - Solution XY Plot menu, should look exactly like the image below.
Then, click Apply in the Axes - Solution XY Plot menu. Now, select X for Axis and select Major Rules and Minor Rules, as shown below.
Next, click Apply in the Axes - Solution XY Plot menu. Close the Axes - Solution XY Plot menu. Now, click Plot in the Solution XY Plot menu. You should obtain the following output.
It is of interest to compare the numerical velocity profile to the velocity profile obtained from the Blasius solution. 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, BlasiusU.xy. Lastly, click Plot in the Solution XY Plot menu. You should then obtain the following figure.
Lastly, select Write to File located under Options in the Solution XY Plot menu. Then, click Write.... When prompted for a filename, enter XVelOutlet.xy and save the file in your working directory.
Mid-Section Velocity Profile
Here, we will plot the variation of the x component of the velocity along a vertical line in the middle of the geometry. In order to create the profile, we must first create a vertical line at x=0.5m, using the Line/Rake tool. First, (Click) Surface < Line/Rake as shown in the following image.
We'll create a straight vertical line from (x0,y0)=(0.5,0) to (x1,y1)=(0.5,0.5). Select Line Tool under Options. Enter x0=0.5, y0=0,x1=0.5, y1=0.5. Enter line1 under New Surface Name. Your Line/Rake Surface menu should look exactly like the following image.
Next, click Create. Now, that the vertical line has been created we can proceed to the plotting. Click on Plots, then double click XY Plot to open the Solution XY Plot menu. In the Solution XY Plot menu, use the settings that were used from the section above, except select line1 under Surfaces and deselect any other geometry sections. Make sure that Write to File is not selected, then click Plot. You should obtain the following output.
Then, return to the Solution XY Plot menu and select both line1 and outlet under Surfaces. Next, click Plot and you should obtain the following figure.
Once again, return to the Solution XY Plot menu, select Write to File, then click Write.... When prompted for a filename, enter XVelProfs.xy and save the file in your working directory.
Pressure Coefficients
In this section we will create contour plots for the pressure coefficients. Before we begin, we must first set the reference values for velocity. In order to do so, first click on Reference Values then set Compute from to inlet, as shown below.
|^CompInlet_Full.png]
Next, click on Graphics and Animations, then double click on Contours, as shown below.
In the Contours menu, set Contours of to Pressure... and set the box below to Pressure Coefficient. Next, select Filled and set Levels to 90. Your Contours menu should look exactly like the following image.
Lastly, click Display in the Contours menu to generate the contour plot. You should obtain the following output.
You can then zoom in to the leading edge of the plate with the wheel mouse button as shown below.
Skin Friction Coefficient
Here, the skin friction coefficient will be plotted as a function of distance along the plate. First, click on Plots, then double click on XY Plot. In the Solution XY Plot menu deselect Write to File, select Position on X Axis, set X to 1 and set Y to 0. Then, set the box located underneath Y Axis Function to Wall Fluxes and set the box below to Skin Friction Coefficient. Next, select plate under Surfaces and deselect any other geometry features. At this point your Solution XY Plot menu should look the same as the following image.
Make sure that for both the x and y axes, that Auto Range is selected. Remember, that you must click Apply to implement the changes you make. Then, click Plot in the Solution XY Plot menu and you should obtain the following output.
It is of interest to compare the numerical skin friction coefficient profile to the skin friction coefficient profile obtained from the Blasius solution. 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, BlasiusSkin.xy. Lastly, click Plot in the Solution XY Plot menu. You should then obtain the following figure.
Lastly, select Write to File located under Options in the Solution XY Plot menu. Then, click Write.... When prompted for a filename, enter SkinFriction.xy and save the file in your working directory.
Drag
Now, we will obtain the drag on the plate. First, click on Report then click on Result Reports..., as shown in the following image.
Next, double click on Forces and click Print in the Force Reports menu. You should then obtain the following output in the command pane.
As one can see from the data above, the plate experiences a drag of approximately 0.008377 Newtons. Furthermore, the data states that the drag coefficient is approximately 0.01675. The drag coefficient is defined by the following equation.
In the case here, the density, velocity and area all have values of 1. Thus, the equation above reduces to the following equation.
The results from ANSYS FLUENT agree with the theory here since the drag coefficient is approximately twice the value of the drag.
Now, save your work in the FLUENT window, then close the FLUENT window.
Go to Step 7: Verification & Validation