[carl_r]

I’m relatively new to OpenFoam but have experience with other commercial CFD packages. I am trying to create a domain with multiple meshed regions using OpenFoam V7 and snappyHexMesh. But am struggling to find the required methodology to do this.

In openFoam v19.12 snappyHexMesh (sHM) allows the use of the command locationsInMesh, however this command does not seem to be available in the openFoamV7 release. Instead OFV7 uses locationInMesh to define a single region. I am able to move to coordinate of this to choose which single region (of the 3 regions) in the domain is meshed.

All the tutorials I have found online show using topoSet and splitMesh functions to sub-divide the mesh into different regions / surfaces. However, these tutorials show simple mesh generated using block mesh, my geometry does not lend itself to this method, I want to be able to define the regions by .stl files.

I can’t use snappyHexMesh to create the mesh before using topoSet and splitMesh, as I can’t get sHM to generate a full mesh domain to split. If I merge my geometry files into one stl, to produce a mesh of the whole domain, then the nodes/elements will not align (will not have been snapped to the surfaces) with the boundaries between the different regions, meaning I won’t be able to split the domain along the stl file boundaries.

How do I create a multi-region mesh in OpenFoam V7 and snappyHexMesh using .stl files? Can this be done?

I have attached an image of a simple case study geometry and the files required to mesh in using blockMesh and snappyHexMesh. These files result in only the leftmost part being meshed. The geometry I want to mesh is more complex, this is a simplified geometry to try and solve this issue.

[simrego]

Hi!


You need closed surfaces for the regions as you can see in this example:
https://github.com/OpenFOAM/OpenFOAM...ppyHexMeshDict
In the refinementSurfaces entry you can define a cellZone for each region.
It is more complicated than in the ESI version where you just tell shm the inisde points, but you can do it in the foundation version too. Good luck!

[carl_r]

Hi,
Thanks for the response. I've tried, but failed to make any progress, my latest files are attached.

I have created a simple geometry. Fluid is in blue and PartA in grey. Currently I can only get PartA meshed.

I did find another tutorial but this one is slightly different in that the external mesh volume is used with separate regions meshed inside. In my case I want to remove the external mesh and keep only the mesh defined inside the .stl files.

https://holzmann-cfd.com/en/openfoam...-snappyhexmesh


I have some questions which I'd be grateful for the answers too:

1) Can the .stl files for PartA and Fluid both be water tight. This would be my preference. Or do i have to delete the surface between Fluid/PartA in one of the files so that there are no duplicate surfaces?

2) Do I still need the locationInMesh variable, if so does it matter which component I specify it in?

3) Are the below definitions correct based on what I'm trying to achieve and is there something missing?

geometry
{
	Fluid_AllSurf.stl {type triSurfaceMesh; name Fluid;}
	PartA_AllSurf.stl {type triSurfaceMesh; name PartA;}
};


castellatedMeshControls
{
    features 
    (
        {file "Fluid_AllSurf.eMesh"; level 1;} 
        {file "PartA_AllSurf.eMesh"; level 1;}
    );
    
    
    refinementSurfaces
    {
        Fluid         // Tried using .stl file name here, No improvement 
        {
            level (1 1);
            faceZone    faceFluid;
            cellZone    cellFluid;
            cellZoneInside inside;     // inside / outside / specified insidePoint
            boundary    internal;
        }

        PartA
        {
            level (1 1);
            faceZone    facePartA;
            cellZone    cellPartA;
            cellZoneInside inside;
            boundary    internal;
        }
        

        locationInMesh (0.02 0.02 -0.01);   // located in PartA
}

[Yann]

Hi Carl,

I didn't run the case cause I don't have OF7 installed right now, but there is a chtMultiRegionFoam tutorial using snappyHexMesh in OF7 : https://github.com/OpenFOAM/OpenFOAM...eHeatExchanger

The process is still the same : defining cellzones for each regions, meshing the whole domain, then using splitMeshRegions to split your initial mesh in one mesh by region.

Removing the external region isn't a big deal: after splitting the mesh, you can simply delete the unwanted regions. Just pay attention to the boundaries, you may need to adjust the boundary types (wall, patch...) depending on your configuration.

I hope this helps,
Yann

[carl_r]

I have made some progress. I have broken my .stl files down into separate surfaces, so that I can define my patches.

I have got to the point where I can generate either a mesh in the two parts with no patches, or the mesh for 1 part including the patches, but not both.

If I include the faceZone, CellZones and cellZoneInside, boundry lines I get both parts meshed. If I don't include them I get only PartA Meshed, but all the patches are correctly defined.


Geometry Definition:

geometry
{
    Fluid.stl
    {
        type triSurfaceMesh;
        regions
        {
            Fluid_Inlet { name Fluid_Inlet; }
            Fluid_Sym   { name Fluid_Sym; }
            Fluid_Env   { name Fluid_Env; }
            Fluid_PartA { name Fluid_PartA; }
        }
    }
    
    PartA.stl
    {
        type triSurfaceMesh;
        regions
        {
            PartA_Inlet { name PartA_Inlet;}
            PartA_Sym   { name PartA_Sym;}
            PartA_Env   { name PartA_Env;}
            PartA_Fluid { name PartA_Fluid;}
        }
    }

RefinementSurfaces:

    refinementSurfaces         // Surface-wise min and max refinement level
    {
        Fluid.stl
        {
            level (1 1);

            regions
            {
                Fluid_Inlet { level (1 1); patchInfo { type patch; }}
                Fluid_Sym   { level (1 1); patchInfo { type patch }}
                Fluid_Env   { level (1 1); patchInfo { type wall; }}
                Fluid_PartA { level (1 1); patchInfo { type wall; }}
            }
       //     faceZone    faceFluid;
       //     cellZone    cellFluid;
       //     cellZoneInside inside;
       //     boundary    internal;
        }

        PartA.stl
        {
            level (1 1);

            regions
            {
                PartA_Inlet { level (1 1); patchInfo { type patch; }}
                PartA_Sym   { level (1 1); patchInfo { type patch }}
                PartA_Env   { level (1 1); patchInfo { type wall; }}
                PartA_Fluid { level (1 1); patchInfo { type wall; }}
            }
        //    faceZone    facePartA;
        //    cellZone    cellPartA;
        //    cellZoneInside inside;
        //    boundary    internal;
        }

How do I generate the patch names and the two volumes?

Am I correct in thinking that this can all be done in sHM, or do I have to do the patch and part definition in topoSet and splitMesh? I feel like i'm getting confused as there are multiple ways of doing the same thing, with each tutorial choosing a different method.

Files attached.
I would appreciate any help given.

[linnemann]

Hi

If you look at the tutorial tutorials/heatTransfer/chtMultiRegionFoam/shellAndTubeHeatExchanger

It will give you an idea of what you need to do.
Basically you need to divide your geometry into "zones" containing a "closed" volume for each zone. The thing you need to do differently is to have the face between the "zones" being in a separate stl with not regions.

On another note snappy is really not the best mesher for you case due to the pointy end.

[MaySea]

Originally Posted by carl_r

I have made some progress. I have broken my .stl files down into separate surfaces, so that I can define my patches.

I have got to the point where I can generate either a mesh in the two parts with no patches, or the mesh for 1 part including the patches, but not both.

If I include the faceZone, CellZones and cellZoneInside, boundry lines I get both parts meshed. If I don't include them I get only PartA Meshed, but all the patches are correctly defined.


Geometry Definition:

geometry
{
    Fluid.stl
    {
        type triSurfaceMesh;
        regions
        {
            Fluid_Inlet { name Fluid_Inlet; }
            Fluid_Sym   { name Fluid_Sym; }
            Fluid_Env   { name Fluid_Env; }
            Fluid_PartA { name Fluid_PartA; }
        }
    }
    
    PartA.stl
    {
        type triSurfaceMesh;
        regions
        {
            PartA_Inlet { name PartA_Inlet;}
            PartA_Sym   { name PartA_Sym;}
            PartA_Env   { name PartA_Env;}
            PartA_Fluid { name PartA_Fluid;}
        }
    }

RefinementSurfaces:

    refinementSurfaces         // Surface-wise min and max refinement level
    {
        Fluid.stl
        {
            level (1 1);

            regions
            {
                Fluid_Inlet { level (1 1); patchInfo { type patch; }}
                Fluid_Sym   { level (1 1); patchInfo { type patch }}
                Fluid_Env   { level (1 1); patchInfo { type wall; }}
                Fluid_PartA { level (1 1); patchInfo { type wall; }}
            }
       //     faceZone    faceFluid;
       //     cellZone    cellFluid;
       //     cellZoneInside inside;
       //     boundary    internal;
        }

        PartA.stl
        {
            level (1 1);

            regions
            {
                PartA_Inlet { level (1 1); patchInfo { type patch; }}
                PartA_Sym   { level (1 1); patchInfo { type patch }}
                PartA_Env   { level (1 1); patchInfo { type wall; }}
                PartA_Fluid { level (1 1); patchInfo { type wall; }}
            }
        //    faceZone    facePartA;
        //    cellZone    cellPartA;
        //    cellZoneInside inside;
        //    boundary    internal;
        }

How do I generate the patch names and the two volumes?

Am I correct in thinking that this can all be done in sHM, or do I have to do the patch and part definition in topoSet and splitMesh? I feel like i'm getting confused as there are multiple ways of doing the same thing, with each tutorial choosing a different method.

Files attached.
I would appreciate any help given.

Hi Carl,

May I ask you how did you separate your .stl file into regions?
I have multiple .stl files forming one terrain surface and I would like to have them as one .stl file with multiple regions.

EDIT: Ok, I got what I wanted using the cat command cat *.stl >> combined.stl. Easier than I thought.

like this:

    Fluid.stl
    {
        type triSurfaceMesh;
        regions
        {
            Fluid_Inlet { name Fluid_Inlet; }
            Fluid_Sym   { name Fluid_Sym; }
            Fluid_Env   { name Fluid_Env; }
            Fluid_PartA { name Fluid_PartA; }
        }

Cheers,
Jan

[quarkz]

Thanks ppl, I got it to work too.

FYI, my stl was created using Pointwise and I can use the different domains to create the stl, which is separated into multi regions. The CAD was imported from Solidworks.

[Patuco]

Hi,

I am having the same problem, I am not able to generate a multiregion mesh with SHM. Could you send or explain how you managed to solve it, please.

Thank you very much,

[Yann]

Hello Patuco,

Your question is too generic, you should rather explain what you tried to do and what problems you are facing.

How to give enough info to get help

[Patuco]

Hello Yann,
The problem I am having is that when I change my stl and the file names of the tutorial sehllandtubeheatexchanger so that everything makes sense and when I launch the simulation it does not generate the mesh, it only generates the blockmesh.

When I change this blockmesh so that it cuts my mesh, it generates the patches, although it does not generate all my simulation zone. But it does not order them as it should even if I have specified it in SHM and many times they are not even patches between regions.

The geometry is very simple, it tells me that there are closed surfaces but in the tutorial also shows that failure and if it generates the mesh.

This is my SnappyHexMesh code:


#includeEtc "caseDicts/mesh/generation/snappyHexMeshDict.cfg"

castellatedMesh on;
snap on;
addLayers off;

geometry
{
shell
{
type triSurfaceMesh;
file "shell.stl";
regions
{
inlet_s { name inlet_s; }
outlet_s { name outlet_s; }
}
}
air
{
type triSurfaceMesh;
file "air.stl";
regions
{
inlet_a { name inlet_a; }
outlet_a { name outlet_a; }
down { name down; }
top { name top; }
laterales { name laterales; }
}
}
solid
{
type triSurfaceMesh;
file "solid.stl";
regions
{
in_wall { name in_wall; }
out_wall { name out_wall; }
}
}

shell_to_solid
{
type triSurfaceMesh;
file "shell_to_solid.stl";
}
air_to_shell
{
type triSurfaceMesh;
file "air_to_shell.stl";
}
};

castellatedMeshControls
{
features
(
);

refinementSurfaces
{
shell
{
level (1 1);

regions
{
inlet_s { level (1 1); patchInfo { type patch; } }
outlet_s { level (1 1); patchInfo { type patch; } }

}
}
air
{
level (1 1);
regions
{
inlet_a { level (1 1); patchInfo { type patch; } }
outlet_a { level (1 1); patchInfo { type patch; } }

}
}
solid
{
level (1 1);
regions
{
in_wall { level (1 1); patchInfo { type wall; } }
out_wall { level (1 1); patchInfo { type wall; } }
}
}

shell_to_solid
{
level (1 1);
faceZone shell_to_solid;
cellZone shell;
mode inside;
}
air_to_shell
{
level (1 1);
faceZone air_to_shell;
cellZone air;
mode inside;
}
}

insidePoint (0 0.008 0.015);

nCellsBetweenLevels 2;

resolveFeatureAngle 15;
}

snapControls
{
implicitFeatureSnap true;
}

addLayersControls
{
layers
{

shell_to_solid
{
nSurfaceLayers 2;
mergeFaces false;
}
air_to_shell
{
nSurfaceLayers 2;
mergeFaces false;
}
}

relativeSizes true;
expansionRatio 1.2;
finalLayerThickness 0.5;
minThickness 1e-3;
}

mergeTolerance 1e-6;

[Yann]

Could you post the log files of snappy and splitMesh?

Are you running the Allmesh.layers or Allmesh.noLayers scripts?
In order to debug your case it would probably be better to use the Allmesh.noLayers as it is simpler and avoid all the extra steps done to deal with layer addition.