6.3.15 Reading Multiple Mesh/Case/Data Files

There may be some cases in which you will need to read multiple mesh files (subdomains) to form your computational domain.

• To solve on a multiblock mesh, generate each block of the mesh in the mesh generator and save it to a separate mesh file.

• For very complicated geometries, it may be more efficient to save the mesh for each part as a separate mesh file.

The mesh node locations need not be identical at the boundaries where two separate meshes meet. ANSYS FLUENT can handle non-conformal mesh interfaces. See Section  6.4 for details about non-conformal mesh boundaries.

There are two ways for reading multiple mesh files in ANSYS FLUENT:

• Using ANSYS FLUENT's ability to read multiple mesh files.

• Using TGrid or tmerge.

Using ANSYS FLUENT's Ability to Read Multiple Mesh Files

ANSYS FLUENT allows you to handle more than one mesh at a time within the same solver settings. This capability of handling multiple meshes saves time, since you can directly read in the different mesh files in ANSYS FLUENT itself without using other tools like TGrid or tmerge.

The steps to take when reading more than one mesh file are:

1.   Read in your first mesh file.

File $\rightarrow$ Read $\rightarrow$ Mesh...

In the Select File dialog box (see Section  2.1.6) (Figure  6.3.1), select the mesh file and click OK.

Figure 6.3.1: The Select File Dialog Box

2.   Read in your second mesh file and append it to the first mesh selected in the first step.

Mesh $\rightarrow$ Zone $\rightarrow$ Append Case File...

In the Select File dialog box (see Section  2.1.6), select the second mesh file and click OK.

3.   (optional). Display your meshes using the Mesh Display dialog box.

General Display...

You will find that the second mesh is appended to the first.

ANSYS FLUENT also allows you to append the data on the mesh. To do that, follow the procedure above. For the second step, use the following menu item:

Mesh $\rightarrow$ Zone $\rightarrow$ Append Case & Data Files...

Select the case file in the Select File dialog box (see Section  2.1.6) (Figure  6.3.1), and click OK. Both the case and data files will be appended.

Reading multiple mesh and data options are available only for serial cases, not for parallel cases.

Using TGrid or tmerge

1.   Generate the mesh for the whole domain in the mesh generator, and save each cell zone (or block or part) to a separate mesh file for ANSYS FLUENT.

If one (or more) of the meshes you wish to import is structured (e.g., a FLUENT 4 mesh file), first convert it to ANSYS FLUENT format using the fl42seg filter described in Section  6.3.13.

2.   Before starting the solver, use either TGrid or the tmerge filter to combine the meshes into one mesh file. The TGrid method is convenient, but the tmerge method allows you to rotate, scale, and/or translate the meshes before they are merged.

• To use TGrid, do the following:

  (a)   Read all of the mesh files into TGrid. When TGrid reads the mesh files, it will automatically merge them into a single mesh.

  (b)   Save the merged mesh file.

  See the TGrid User's Guide for information about reading and writing files in TGrid.

• To use the tmerge filter, do the following before starting ANSYS FLUENT:

  (a)   For 3D problems, type utility tmerge -3d. For 2D problems, type utility tmerge -2d.

  (b)   When prompted, specify the names of the input files (the separate mesh files) and the name of the output file in which to save the complete mesh. Be sure to include the .msh extension.

  (c)   For each input file, specify scaling factors, translation distances, and rotation information.

  For information about the various options available when using tmerge, type utility tmerge -h.

3.   Read the combined mesh file into the solver in the usual manner (using the File/Read/Mesh... menu item).

For a conformal mesh, if you do not want a boundary between the adjacent cell zones, use the Fuse Face Zones dialog box to fuse the overlapping boundaries (see Section  6.8.3). The matching faces will be moved to a new zone with a boundary type of interior. If all faces on either or both of the original zones have been moved to the new zone, the original zone(s) will be discarded.

If you are planning to use sliding meshes, or if you have non-conformal boundaries between adjacent cell zones, do not combine the overlapping zones. Instead, change the type of the two overlapping zones to interface (as described in Section  6.4).

In this example, scaling, translation, or rotation is not requested. Hence you can simplify the inputs to the following:

user@mymachine:>
utility tmerge -2d

Starting /Fluent.Inc/utility/tmerge2.1/ultra/tmerge_2d.2.1.13

Append 2D grid files.
tmerge2D Fluent Inc, Version 2.1.11

 Enter name of grid file (ENTER to continue) : 
my1.msh


 x,y scaling factor, eg. 1 1             : 
1 1


 x,y translation, eg. 0 1                : 
0 0


 rotation angle (deg), eg. 45            : 
0


 Enter name of grid file (ENTER to continue) : 
my2.msh


 x,y scaling factor, eg. 1 1             : 
1 1


 x,y translation, eg. 0 1                : 
0 0


 rotation angle (deg), eg. 45            : 
0


 Enter name of grid file (ENTER to continue) : 
<Enter>


 Enter name of output file               : 
final.msh


Reading...
  node zone: id 1, ib 1, ie 1677, typ 1
  node zone: id 2, ib 1678, ie 2169, typ 2
      .
      .
      .
done.
Writing...
  492 nodes, id 1, ib 1678, ie 2169, type 2.
  1677 nodes, id 2, ib 1, ie 1677, type 1.
      .
      .
      .
done.
Appending done.