[Isaac]

Hello,
The actual case I am trying to simulate is different than below. But this is a simple enough example to explain what I am trying to do and hopefully get some help. Before I begin, I want to assure you that I have done some extensive searching on forums and other places and I have tried many of the things that have been suggested (to the best of my comprehension) and not been successful. So I am hoping someone can be a little more specific in their instructions.
A schematic of what I am trying to simulate is attached – a pipe with an elbow with two thin plates acting like baffles. I created this mesh in a third-party software (Gambit to be precise) and save it as a Fluent mesh file (.msh).


I convert this file into OpenFoam using the command FluentMeshToFoam pipeBafflesOF.msh
The mesh converts just fine except that, as most of you would know, the baffles don't get converted because they are considered “internal” faces with mesh on both sides. I get the following messages:

Building boundary and internal patches.
Creating patch 0 for zone: 3 start: 1 end: 101 type: wall name: wall-Pipe
Creating patch 1 for zone: 4 start: 102 end: 109 type: pressure-outlet name: Outlet
Creating patch 2 for zone: 5 start: 110 end: 117 type: velocity-inlet name: Inlet
Creating patch 3 for zone: 6 start: 118 end: 123 type: wall name: wall-baffle2
Creating patch 4 for zone: 7 start: 124 end: 134 type: wall name: wall-baffle1
Creating patch 5 for zone: 9 start: 135 end: 1542 type: interior name: default-interior
Creating patch for front and back planes

Adding new patch wall-Pipe of type wall as patch 0
Adding new patch Outlet of type patch as patch 1
Adding new patch Inlet of type patch as patch 2
Patch wall-baffle2 is internal to the mesh and is not being added to the boundary.
Patch wall-baffle1 is internal to the mesh and is not being added to the boundary.
Patch default-interior is internal to the mesh and is not being added to the boundary.
Adding new patch frontAndBackPlanes of type empty as patch 3

Writing mesh... to "constant/polyMesh" done.


End

As you can see the two baffles wall-baffle1 and wall-baffle2 are not added to the patch list. Now, this is where I struggle. There is one tutorial on youtube for something similar where the mesh is cerated used gmsh. It looks like in that case, the patches are added for these thin walls but not recognized as boundaries. Therefore when you run the createBafflesDict, the boundaries are created. In my case, if I run createBafflesDict, it creates a new patch with zero faces. It does not show up as a boundary in paraView.

baffles
{
wall-baffles
{
type faceZone;
zoneName wall-baffles;

patches
{
master
{
name wall-baffles;
type wall;
}
slave
{
${..master}
}
}
}
}

I then tried to run the createPatchDict. For this I modified the boundary file and added the following patch information manually based on the start faces that was output during conversion.

wall-baffle1
{
type patch;
nFaces 11;
startFace 124;
}
wall-baffle2
{
type patch;
nFaces 11;
startFace 118;
}

Then my createPatchDict file looked something like this:

patches
(
{
name wall-baffle1;
patchInfo
{
type wall;
}
constructFrom patches;
patches (wall-baffle1);
}
{
name wall-baffle2;
patchInfo
{
type wall;
}
constructFrom patches;
patches (wall-baffle2);
}
);

But I get an error. I don't think the start faces for the boundaries are correct. I am not sure how to proceed from here on.
Can any of you please point me in the right direction in a little specific detail. I am really stuck with my problem because of this.
Thank you for your help.

Isaac

[Isaac]

I think I found a solution of sorts for those who may find it useful in the future. If anybody sees any errors or issues in my implementation, I will be open to them.

Following are some of the steps:
1. The faces (boundaries) should be named when the mesh is created.
2. When converting the mesh, explicitly write out sets. For example:
fluentMeshToFoam <filaname.msh> -writeSets
This writes out the sets to a folder called sets under constant -->polymesh-->sets
You will see all the boundaries and associated faces in this folder.
3. Now, set the topology for the thin walls. For this you need to modify the topoSetDict file under the System folder. An example of this file will look as follows:

actions
(
{
name wall-Baffle1;
type faceZoneSet;
action new;
source setToFaceZone;
sourceInfo
{
faceSet wall-baffle1;
}
}
{
name wall-Baffle2;
type faceZoneSet;
action new;
source setToFaceZone;
sourceInfo
{
faceSet wall-baffle2;
}
}
);

The type faceZoneSet is telling the program to look for a set with the name shown under it.
The command for this is :
topoSet -dict system/topoSetDict

4. This will set the topology for these boundaries.
5. Next, convert these boundaries to baffles using the dictionary createBafflesDict. Modify the controlBafflesDict file similar to the following example:

internalFacesOnly true;

baffles
{
wall-Baffle1
{
type faceZone;
zoneName wall-Baffle1;

patches
{
master
{
name wall-Baffle1;
type wall;
}
slave
{
${..master}
}
}
}

wall-Baffle2
{
type faceZone;
zoneName wall-Baffle2;

patches
{
master
{
name wall-Baffle2;
type wall;
}
slave
{
${..master}
}
}
}
}

Run the following command:
createBaffles -dict system/createBafflesDict -overwrite

This will add the patches in the boundary file.

6. Now, set the correct boundary conditions and the problem is ready to be solved.

Note that this is good for Flow Modeling. Not sure about setting Heat Transfer conduction across this thin wall.