6.8.3 Fusing Face Zones

The face-fusing utility is a convenient feature that can be used to fuse boundaries (and merge duplicate nodes and faces) created by assembling multiple mesh regions. When the domain is divided into subdomains and the mesh is generated separately for each subdomain, you will combine the subdomains into a single file before reading the mesh into the solver. (See Section  6.3.15 for details.) This situation could arise if you generate each block of a multiblock mesh separately and save it to a separate mesh file. Another possible scenario is that you decided, during mesh generation, to save the mesh for each part of a complicated geometry as a separate part file. (Note that the mesh node locations need not be identical at the boundaries where two subdomains meet; see Section  6.4 for details.)

The Fuse Face Zones dialog box (Figure  6.8.5) allows you to merge the duplicate nodes and delete these artificial internal boundaries.

Mesh $\rightarrow$ Fuse...

Figure 6.8.5: The Fuse Face Zones Dialog Box

The boundaries on which the duplicate nodes lie are assigned zone ID numbers (just like any other boundary) when the mesh files are combined, as described in Section  6.3.15. You need to keep track of the zone ID numbers when tmerge or TGrid reports its progress or, after the complete mesh is read in, display all boundary mesh zones and use the mouse-probe button to determine the zone names (see Section  29.3 for information about the mouse button functions).

Inputs for Fusing Face Zones

The steps for fusing face zones are as follows:

1.   Select the zones to be fused in the Zones list.

2.   Click the Fuse button to fuse the selected zones.

If all of the appropriate faces do not get fused using the default Tolerance, you should increase it and attempt to fuse the zones again. (This tolerance is the same as the matching tolerance discussed in Section  6.8.4.) The Tolerance should not exceed 0.5, or you may fuse the wrong nodes.

When fusing face zones using the GUI, ANSYS FLUENT automatically assigns a new name to the fused interface zone. If you would like to preserve the original name of one of the face zones being fused, you can use the mesh/modify-zones/fuse-face-zones text command, as shown in the following example.

/mesh/modify-zones> fuse-face-zones

()
Zone to fuse(1) [()] top

Zone to fuse(2) [()] bottom.1

Zone to fuse(3) [()] <Enter>


  all 378 faces matched for zones 3 and 12.
    fusing created new thread, interior-18.
The fused zone name: (automatic bottom.1 top) 
Enter name [automatic] top

 Name of zone 18 is changed into top.

 Fused list of zones.

Remember to save a new case file (and a data file, if data exist) after fusing faces.

Fusing Zones on Branch Cuts

Meshes imported from structured mesh generators or solvers (such as FLUENT 4) can often be O-type or C-type meshes with a reentrant branch cut where coincident duplicate nodes lie on a periodic boundary. Since ANSYS FLUENT uses an unstructured mesh representation, there is no reason to retain this artificial internal boundary. (Of course, you can preserve these periodic boundaries and the solution algorithm will solve the problem with periodic boundary conditions.)

To fuse this periodic zone with itself, you must first slit the periodic zone, as described in Section  6.8.5. This will create two symmetry zones that you can fuse using the procedure above.

Note that if you need to fuse portions of a non-periodic zone with itself, you must use the mesh/modify-zones/fuse-face-zones text command.

mesh $\rightarrow$ modify-zones $\rightarrow$ fuse-face-zones

This command will prompt you for the name or ID of each zone to be fused. (You will enter the same zone twice.) To change the node tolerance, use the mesh/modify-zones/
matching-tolerance text command.