mergeTwoMesh.md

Merge two different mesh files

This tutorial shows how to merge two mesh files genreated by two different softwares.

--------- 
|       |  
|       ----   ---------------
|    A     |   |      B      |
|          |   |             |
-----------    ---------------
           ^   ^
         interface

For example, a body can be divided to part A and part B. They are connected through the interface: inter-A and inter-B.

Use Fluent meshing to generate poly-hexcore mesh for part A. Use ICEM to generate struct hexal mesh for part B. The interface of A and B have different mesh. (Version 22R1)

1. Combine two mesh sets

• Fluent <solution mode> -> Read mesh A
• Domain -> Zones -> Append (append case file) -> Select part B mesh file -> Click ok -> ignore the warnings
• Domain -> Zone -> Combine (merge) -> fluid (select two fluid zones) -> Merge
• File -> Write -> Case, for example test.cas

2. Get mesh from the case file

• Fluent <meshing mode>
• File -> Read (case) -> select test.cas
• Use TUI to export mesh file

Meshing> file
Meshing/file> file-format
Write binary files? [yes] no
Meshing/file> write-mesh test.msh

3. Convert the merged mesh to OpenFOAM

fluen3DMeshToFoam test.msh -scale 0.001

Edit the constant/boundary file, change inter-A and inter-B settings to:

    inter-A
    {
        nFaces          xxxxxx;
        startFace       xxxxxx;

        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        matchTolerance  0.0001;
        neighbourPatch  inter-B;
        transform       noOrdering;

    }
    inter-B
    {
        nFaces          xxxxxx;
        startFace       xxxxxx;

        type            cyclicAMI;
        inGroups        1(cyclicAMI);
        matchTolerance  0.0001;
        neighbourPatch  inter-B;
        transform       noOrdering;
    }

Boundary conditions for any variables:

    inter-A
    {
        type            cyclicAMI;
    }
    inter-B
    {
        type            cyclicAMI;
    }