Step 3: General Settings

  Select General in the navigation pane to perform the mesh-related activities and to choose a solver.

General

1.   Check the mesh.

General Check

   ANSYS FLUENT will report the results of the mesh check in the console.

Mesh Check
 
 Domain Extents:
   x-coordinate: min (m) = -8.000000e+000, max (m) = 8.000000e+000
   y-coordinate: min (m) = -9.134633e+000, max (m) = 8.000000e+000
   z-coordinate: min (m) = 0.000000e+000, max (m) = 2.000000e+000
 Volume statistics:
   minimum volume (m3): 5.098261e-004
   maximum volume (m3): 2.330738e-002
     total volume (m3): 1.607154e+002
 Face area statistics:
   minimum face area (m2): 4.865882e-003
   maximum face area (m2): 1.017924e-001
 Checking number of nodes per cell.
 Checking number of faces per cell.
 Checking thread pointers.
 Checking number of cells per face.
 Checking face cells.
 Checking cell connectivity.
 Checking bridge faces.
 Checking right-handed cells.
 Checking face handedness.
 Checking face node order.
 Checking element type consistency.
 Checking boundary types:
 Checking face pairs.
 Checking periodic boundaries.
 Checking node count.
 Checking nosolve cell count.
 Checking nosolve face count.
 Checking face children.
 Checking cell children.
 Checking storage.
Done.

Note:   The minimum and maximum values may vary slightly when running on different platforms. The mesh check will list the minimum and maximum $x$ and $y$ values from the mesh in the default SI unit of meters. It will also report a number of other mesh features that are checked. Any errors in the mesh will be reported at this time. Ensure that the minimum volume is not negative, since ANSYS FLUENT cannot begin a calculation when this is the case.

2.   Scale the mesh.

General Scale...

(a)   Make sure that Convert Units is selected in the Scaling group box.

(b)   Select in from the Mesh Was Created In drop-down list by first clicking the down-arrow button and then clicking the in item from the list that appears.

(c)   Click Scale to scale the mesh.

Be sure to click the Scale button only once.

   Domain Extents will continue to be reported in the default SI unit of meters.

(d)   Select in from the View Length Unit In drop-down list to set inches as the working unit for length.

(e)   Confirm that the domain extents are as shown in the previous dialog box.

(f)   Close the Scale Mesh dialog box.

  The mesh is now sized correctly and the working unit for length has been set to inches.

Note:   Because the default SI units will be used for everything except length, there is no need to change any other units in this problem. The choice of inches for the unit of length has been made by the actions you have just taken. If you want a different working unit for length, other than inches (e.g., millimeters), click Units... in the General task page and make the appropriate change, in the Set Units dialog box.

3.   Check the mesh.

General Check

Note:   It is a good idea to check the mesh after you manipulate it (i.e., scale, convert to polyhedra, merge, separate, fuse, add zones, or smooth and swap). This will ensure that the quality of the mesh has not been compromised.

4.   Retain the default settings in the Solver group box of the General task page.