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 Fluent. For details, see Reading Multiple Mesh/Case/Data Files. 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 Non-Conformal Meshes for details.)
The Fuse Face Zones dialog box (Figure 5.70: The Fuse Face Zones Dialog Box) allows you to merge the duplicate nodes and delete these artificial internal boundaries.
Setting Up Domain → Zones → Combine → Fuse...
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 Reading Multiple Mesh/Case/Data Files. You need to keep track of
the zone ID numbers when tmerge or the meshing
mode of Fluent 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 Controlling the Mouse Button Functions for information about the mouse
button functions). Alternatively, you can specify a name for the fused
zone.
The steps for fusing face zones are as follows:
Select the zones to be fused in the Zones list.
Important: When using the Fuse Face Zone utility, each of the selected face zones must be fused in its entirety with another face zone having the same connectivity. Partial fusing of face zones is not supported.
(Optional) If you would like to specify a name for the fused zone rather than use an automatically generated name (for instance, to preserve the original name of one of the face zones), disable Use default name for new fused zone and enter the desired name.
Click the 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 Creating Conformal Periodic Zones.) The Tolerance should not exceed 0.5, or you may fuse the wrong nodes.
You can also fuse zones using 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) [()]w1.topZone to fuse(2) [()]w3Zone to fuse(3) [()][Enter]Choose from list (automatic w3 w1.top) or pick your own Enter the fused zone name: [automatic]w3Name of zone 14 is changed into w3. Fused list of zones successfully.
Important: Remember to save a new case file (and a data file, if data exists) after fusing faces.
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. (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 Slitting Periodic Zones. 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 → modify-zones → 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.