5.3.18. 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.

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 Non-Conformal Meshes for details about non-conformal mesh boundaries.

There are three ways of reading multiple mesh files in ANSYS Fluent:

5.3.18.1. Reading Multiple Mesh Files via the Solution Mode of Fluent

The solution mode of 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 and start setting up the solution, without having to switch over from meshing mode or employ another tool such as tmerge.

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

  1. Read in your first mesh file.

     File → Read → Mesh...

    In The Select File Dialog Box (Figure 5.24: The Select File Dialog Box), select the mesh file and click OK.

    Figure 5.24:  The Select File Dialog Box

    The Select File Dialog Box

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

     Setting Up Domain → Zones → Append → Append Case File...

    In The Select File Dialog Box, select the second mesh file and click OK.

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

     Setup →   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 ribbon tab item:

 Setting Up Domain → Zones → Append → Append Case & Data Files...

Select the case file in The Select File Dialog Box (Figure 5.24: The Select File Dialog Box), and click OK. Both the case and data files will be appended.


Important:  Review your case setup after appending multiple mesh and/or data files before proceeding with the calculation.


5.3.18.2. Reading Multiple Mesh Files via the Meshing Mode of Fluent

  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 Fluent.


    Important:  If one (or more) of the meshes you want to import is structured (for example, a FLUENT 4 mesh file), first convert it to ANSYS Fluent format using the fl42seg filter described in FLUENT 4 Case Files.


  2. In the meshing mode of Fluent, combine the meshes into one mesh file.

    1. Read all of the mesh files. As the mesh files are read, they will be automatically merged into a single mesh.

    2. Save the merged mesh file.

    See the Fluent Meshing User’s Guide for information about reading and writing files in meshing mode.

  3. Switch over to the solution mode of Fluent or read the combined mesh file into a new session using the File/Read/Mesh... ribbon tab 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. For details, see Fusing Face Zones. The matching faces will be moved to a new zone with a boundary type of interior and the original zone(s) will be discarded.


Important:  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 Non-Conformal Meshes).


5.3.18.3. Reading Multiple Mesh Files via 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.


    Important:  If one (or more) of the meshes you want to import is structured (for example, a FLUENT 4 mesh file), first convert it to ANSYS Fluent format using the fl42seg filter described in FLUENT 4 Case Files.


  2. Before launching Fluent, use the tmerge filter to combine the meshes into one mesh file. The tmerge method allows you to rotate, scale, and/or translate the meshes before they are merged. Note that the tmerge filter allows you to merge large meshes with very low memory requirement.

    1. For 3D problems, type utility tmerge -3d. For 2D problems, type utility tmerge -2d.

    2. 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.

    3. 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 solution mode of Fluent in the usual manner (using the File/Read/Mesh... ribbon tab 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. For details, see Fusing Face Zones. The matching faces will be moved to a new zone with a boundary type of interior and the original zone(s) will be discarded.


Important:  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 Non-Conformal Meshes).


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 /ansys_inc/v182/fluent/utility/tmerge18.2/lnamd64/tmerge_2d.18.2.0
 
 Append 2D grid files.
 tmerge2D ANSYS Inc, stream

 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.

Release 18.2 - © ANSYS, Inc. All rights reserved.