CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

Internal Interface in mesh imported

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 10, 2019, 13:55
Default Internal Interface in mesh imported
  #1
New Member
 
Hernan
Join Date: Jul 2015
Posts: 3
Rep Power: 8
hernanrmz is on a distinguished road
Hello Foamers!

I want to define an internal interface in a fluid region of an imported mesh from Star-ccm+. This is because I used different mesh operations in Star-ccm+ and creates internal interfaces.

I have a very simple case (Image attached). In this case, the internal interface makes no sense, but in other cases it does.

When I run ccm26ToFoam the boundary file generated is this:

Code:
6
(
    Wall-1
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          1800;
        startFace       88014;
    }
    Int-1
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          518;
        startFace       89814;
    }
    Inlet
    {
        type            patch;
        nFaces          518;
        startFace       90332;
    }
    Wall-2
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          1800;
        startFace       90850;
    }
    Outlet
    {
        type            patch;
        nFaces          518;
        startFace       92650;
    }
    Int-2
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          518;
        startFace       93168;
    }
)
In this post simple problem with internal faces Boundary condition solves a similar problem, but they solved it manipulating the mesh in gambit...

I used "stitchMesh Int-1 Int-2" but it doesn't work, maybe I used wrong...

stitchMesh description: "Merge the faces on the specified patches (if geometrically possible) so the faces become internal."

Anyone have an idea?

Thanks!!
Attached Images
File Type: png Mesh_Starccm.PNG (162.9 KB, 13 views)

Last edited by hernanrmz; October 11, 2019 at 10:35.
hernanrmz is offline   Reply With Quote

Old   October 11, 2019, 11:04
Default
  #2
New Member
 
Hernan
Join Date: Jul 2015
Posts: 3
Rep Power: 8
hernanrmz is on a distinguished road
Hello Foamers!

I just solved! "stitchMesh" is the utility I need

The steps to convert a Star-CCM+ mesh with internal interfaces are:

1. ccm26ToFoam mesh.ccm (you need to install ccm26ToFoam library)
2. The boundary file generated is this:

Code:
6
(
    Wall-1
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          1800;
        startFace       88014;
    }
    Int-1
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          518;
        startFace       89814;
    }
    Inlet
    {
        type            patch;
        nFaces          518;
        startFace       90332;
    }
    Wall-2
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          1800;
        startFace       90850;
    }
    Outlet
    {
        type            patch;
        nFaces          518;
        startFace       92650;
    }
    Int-2
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          518;
        startFace       93168;
    }
)
where "Int-1" and "Int-2" are the faces that define the internal interface. Note that nFaces is 518.

3. You need to define the boundary conditions for the Int-1 and Int-2 in the 0 Files. In this case U and p files.

U file:

Code:
boundaryField
{
    Inlet
    {
        type            fixedValue;
        value           uniform (0.01 0 0);
    }

    Outlet
    {
        type            zeroGradient;
    }
    Wall-1
    {
        type            noSlip;
    }
    Wall-2
    {
        type            noSlip;
    }
   Int-1 
    {
        type            zeroGradient;
    }
   Int-2 
    {
        type            zeroGradient;
    }
}
You can put any condition, it just for preventing an error when you run the stitchMesh. I define the same condition for p file.

If you run checkMesh, you can see that you have 2 regions:

Code:
   *Number of regions: 2
    The mesh has multiple regions which are not connected by any face.
4. Run the stitchMesh utility:

Code:
stitchMesh Int-1 Int-2
This will generate a time folder with the boundary files (U, p) and the polymesh folder.

5. Delete the old polymesh and copy the new one:

Code:
rm -rv constant/polyMesh/
cp -rv 1/polyMesh/ constant/
rm -rv 1
If you run checkMesh again, it tells you that you have one region:

Code:
Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).
The boundary file now have nFaces=0:

Code:
    Int-1
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          0;
        startFace       90332;
6. Now you can delete the Int-1 and Int-2 from boundary file, and from BC files (p, U), or you can just run.

7.
Code:
simpleFoam
Attached Images
File Type: jpg Tubo-Paraview.jpg (32.4 KB, 13 views)
hernanrmz is offline   Reply With Quote

Reply

Tags
internal mesh, star-ccm+

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Radiation in semi-transparent media with surface-to-surface model? mpeppels CFX 11 August 22, 2019 07:30
Frozen Rotor 1:1 Mesh Connection pharley CFX 5 January 31, 2013 16:15
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 11:45
engrid: Internal volume mesh becoming coarser during boundayr layer addition Arnoldinho OpenFOAM 1 January 22, 2011 04:31
Mesh motion applied to an internal interface lr103476 OpenFOAM Running, Solving & CFD 6 March 12, 2008 21:07


All times are GMT -4. The time now is 04:18.