Step 10: Comparing the Results of Both Systems in ANSYS CFD-Post

In this step, you will create a new Results system in ANSYS Workbench, and use that system to compare the solutions from each of the two ANSYS FLUENT-based fluid flow analysis systems in ANSYS CFD-Post at the same time.

1.   Create a Results system.

In ANSYS Workbench, drag a Results system from the Component Systems section of the Toolbox and drop it into the Project Schematic, next to the fluid flow systems.

Figure 1.37: The New Results System in the Project Schematic

2.   Add the solutions of each of the systems to the Results system.

  

(a)   Select the Solution cell in the first Fluid Flow analysis system (cell A5) and drag it over the Results cell in the Results system (cell C2). This creates a transfer data connection between the two systems.

Figure 1.38: Connecting the First Fluid Flow System to the New Results System

(b)   Select the Solution cell in the second Fluid Flow analysis system (cell B5) and drag it over the Results cell in the Results system (cell C2). This creates a transfer data connection between the two systems.

Figure 1.39: Connecting the Second Fluid Flow System to the New Results System

3.   Open ANSYS CFD-Post to compare the results of the two fluid flow systems.

Now that the two fluid flow systems are connected to the Results system, double-click the Results cell in the Results system (cell C2) to open ANSYS CFD-Post. Within ANSYS CFD-Post, both geometries are displayed side by side.

Figure 1.40: ANSYS CFD-Post with Both Fluid Flow Systems Displayed

(a)   Re-orient the display.

In each view, click the blue Z axis on the axis triad in the bottom right hand corner of the graphics display to orient the display so that the view is of the front of the elbow geometry.

Alternatively, you can select the synchronization tool ( ) in the 3D Viewer Toolbar to synchronize the views, so that when you re-orient one view, the other view is automatically updated.

(b)   Display filled contours of velocity magnitude on the symmetry plane.

i.   Insert a contour object.

Insert $\rightarrow$ Contour

  This displays the Insert Contour dialog box.

ii.   Keep the default name of the contour ( Contour 1) and click OK to close the dialog box.

  This displays the Details of Contour 1 view below the Outline view in ANSYS CFD-Post. This view contains all of the settings for a contour object.

iii.   In the Geometry tab, select fluid in the Domains list.

iv.   Select symmetry in the Locations list.

v.   Select Velocity in the Variable list.

vi.   Click Apply.

   In each view, the velocity contours are displayed.

Figure 1.41: ANSYS CFD-Post Displaying Velocity Contours for Both Geometries

(c)   Display filled contours of temperature on the symmetry plane.

i.   Deselect the Contour 1 object under User Location and Plots in ANSYS CFD-Post to hide the first contour display.

ii.   Insert another contour object.

Insert $\rightarrow$ Contour

  This displays the Insert Contour dialog box.

iii.   Keep the default name of the contour ( Contour 2) and click OK to close the dialog box.

  This displays the Details of Contour 2 view below the Outline view in ANSYS CFD-Post. This view contains all of the settings for a contour object.

iv.   In the Geometry tab, select fluid in the Domains list.

v.   Select symmetry in the Locations list.

vi.   Select Temperature in the Variable list.

vii.   Click Apply.

   In each view, the temperature contours are displayed.

Figure 1.42: ANSYS CFD-Post Displaying Temperature Contours for Both Geometries

4.   Close the ANSYS CFD-Post application.

5.   Save the elbow-workbench project in ANSYS Workbench.

6.   View the files generated by ANSYS Workbench.

View the files associated with your project using the Files view.

View $\rightarrow$ Files

Figure 1.43: ANSYS Workbench Displaying the Files View for the Project After Viewing the Combined Results in ANSYS CFD-Post

Note the addition of the Results system and its corresponding files.