Step 5: Displaying Results in ANSYS FLUENT and ANSYS CFD-Post

1.   Display results in ANSYS FLUENT.

With ANSYS FLUENT still running, you can perform a simple evaluation of the velocity and temperature contours on the symmetry plane. Later, you will use ANSYS CFD-Post (from within ANSYS Workbench) to perform the same evaluation.

(a)   Display filled contours of velocity magnitude on the symmetry plane (Figure  1.21).

Graphics and Animations Contours Set Up...

   You can also double-click a list item in order to open the corresponding dialog box.

i.   Enable Filled in the Options group box.

ii.   Make sure that Node Values is enabled in the Options group box.

iii.   Select Velocity... and Velocity Magnitude from the Contours of drop-down lists.

iv.   Select symmetry from the Surfaces selection list.

v.   Click Display to display the contours in the active graphics window.

Figure 1.21: Velocity Distribution Along Symmetry Plane

(b)   Display filled contours of temperature on the symmetry plane (Figure  1.22).

Graphics and Animations Contours Set Up...

i.   Select Temperature... and Static Temperature from the Contours of drop-down lists.

ii.   Click Display and close the Contours dialog box.

Figure 1.22: Temperature Distribution Along Symmetry Plane

(c)   Close the ANSYS FLUENT application.

File $\rightarrow$ Close FLUENT

Note that the ANSYS FLUENT case and data files are automatically saved when you exit ANSYS FLUENT and return to ANSYS Workbench.

(d)   View the files generated by ANSYS Workbench.

View $\rightarrow$ Files

Figure 1.23: ANSYS Workbench Displaying the Files View for the Project After Exiting ANSYS FLUENT

Note the addition of the compressed ANSYS FLUENT case file ( FFF-1.cas.gz) and corresponding data file ( FFF-1-00231.dat.gz) to the list of files. Also note that the name of the data file is based on the number of iterations, so your data file name may be different.

2.   Display results in ANSYS CFD-Post.

(a)   Start ANSYS CFD-Post.

In the ANSYS Workbench Project Schematic, double-click the Results cell in the elbow fluid flow analysis system (cell A6). This displays the ANSYS CFD-Post application. You can also right-click on the Results cell to display the context menu where you can select the Edit option.

  This displays the ANSYS CFD-Post application with the elbow geometry already loaded (displayed in outline mode). Note that ANSYS FLUENT results (e.g., case and data files) are also automatically loaded into ANSYS CFD-Post.

Figure 1.24: The Elbow Geometry Loaded into ANSYS CFD-Post

(b)   Re-orient the display.

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.

(c)   Display filled contours of velocity magnitude on the symmetry plane (Figure  1.25).

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.

Figure 1.25: Velocity Distribution Along Symmetry Plane

(d)   Display filled contours of temperature on the symmetry plane (Figure  1.26).

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

ii.   Insert a 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.

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.

Figure 1.26: Temperature Distribution Along Symmetry Plane

3.   Close the ANSYS CFD-Post application.

Note that the ANSYS CFD-Post state files are automatically saved when you exit ANSYS CFD-Post and return to ANSYS Workbench.

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

5.   View the files generated by ANSYS Workbench.

View $\rightarrow$ Files

Figure 1.27: ANSYS Workbench Displaying the Files View for the Project After Viewing Results in ANSYS CFD-Post

Note the addition of the ANSYS CFD-Post state file ( elbow.cst) to the list of files. For more information about ANSYS CFD-Post (and the files associated with it), see the ANSYS CFD-Post documentation.