Numerical 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.) Click on z axis in the triad (at the bottom right of the graphics window) to get the view along the z-axis.

...

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.

You can save the image to a file using the camera icon highlighted below or using the Snipping Tool in Windows 7 (you can search for it under Start > Programs).

...

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.

...

Name it "Centerline" and click OK. On the lower left panel, you will see Details of Centerline. Enter the start and end locations of the line and the sampling frequency. Click Apply.

You will see centerline created under User Locations and Plots.

Insert > Chart 
Please name this chart "Centerline Temperature". You will see Details of Centerline Temperature appear on the lower left.

We'll go through the tabs in the menu to specify the plot that we want. Select the General tab and name the chart "Temperature Variation along Pipe Axis".

Select the Data Series tab. Change Name and Location.

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 axial position on the "x-axis" of the chart.

Click on X Axis tab. Next to Variable, choose X.

Click on Y Axis tab. Next to Variable, choose Temperature.

Click Apply. You will see Centerline Temperature created under Report in the Outline tab.

...

Name it "Wall"  (with capital W; otherwise you'll get a conflict with a reserved name). On the lower left panel, you will see Details of Wall. Enter the start and end locations of the line and the sampling frequency. Click Apply.

You will see wall created under User Locations and Plots.

Insert > Chart

Name this chart "Wall Temperature". You will see Details of Wall Temperature appear on the lower left panel.

Select the General tab and name the chart "Wall Temperature".

Select Data Series tab. Change the name of the first data series to FLUENT. Under Data Source, specify Wall as Location.

As before, specify x-axis variable to be X (i.e. axial length along the pipe).

Specify y-axis variable to be Temperature. Click Apply. You should see the following plot.

...

First, create the line at x=1.83 m.

Insert > Location > Line

Name it "x183" and click OK. Enter the following coordinates (0.0294 m is the pipe radius).

Point 1 (1.83, 0, 0)
Point 2 (1.83, 0.0294, 0)

Enter 100 for Samples. Click Apply.

Similarly create lines at x=4.27 m and x=6.045 m.

...

Name this chart "Axial Velocity Profiles".

Select the General tab and name the chart "Axial Velocity Profiles".

Select Data Series tab. Change the name of the first data series to x=1.83 m. Under Data Source, specify x183 as Location.

Add a new data series by clicking on the "New" icon as shown below and repeat the above steps but for x=4.27 m.

...

Add a third data series by clicking on the "New" icon and repeating the steps for x=6.045 m. You should then have three items in the Data Series tab.

Specify x-axis variable: Velocity u

Specify y-axis variable: Y

Complete the plot. Here's what we get.

...

Change the title and x-axis variable (to Temperature). Click Apply. Here's what we get.

This plot shows that:

...