[Vishsel]

Hi all,

I am new to Openfoam. Actually I have 5 fluid domains. I exported the mesh for fluid domains individually from ansys mesh and i need to create the interface in between the fluid domains.

My question is, In openfoam, how to write a masterCase and slaveCase for 5 fluid domains in mergeMeshes command ?

To merge two fluid domains into 1, we can use mergeMeshes masterCase slaveCase and how to write for merging of 5 fluid domains into 1 ?


Thankyou in advance.

[Antimony]

Hi,

I don't think there is a way to merge all 5 together. You have to go sequentially if I am not mistaken.

You merge meshes 1 & 2 (let us say the merged is called mesh12). Then you merged mesh12 with mesh3 to get mesh123. You merge mesh123 with mesh4 to get mesh1234. And finally you merge mesh1234 with mesh5 to get the complete merged mesh12345.

Hope this helps.

Cheers,
Antimony

[Vishsel]

Originally Posted by Antimony

Hi,

I don't think there is a way to merge all 5 together. You have to go sequentially if I am not mistaken.

You merge meshes 1 & 2 (let us say the merged is called mesh12). Then you merged mesh12 with mesh3 to get mesh123. You merge mesh123 with mesh4 to get mesh1234. And finally you merge mesh1234 with mesh5 to get the complete merged mesh12345.

Hope this helps.

Cheers,
Antimony

Hi Antimony,

Thanks for your quick response. It's working perfectly.

But interfaces are not created, and every interior faces in the boundary are taken as wall as mentioned below.

15
(
    massflow-inlet
    {
        type            patch;
        nFaces          715;
        startFace       12137752;
    }
    wall-inlet-pipe
    {
        type            wall;
        inGroups        1(wall);
        nFaces          4928;
        startFace       12138467;
    }
    int-pipe-tube-in-1
    {
        type            wall;
        inGroups        1(wall);
        nFaces          715;
        startFace       12143395;
    }
    wall-inlet-tank
    {
        type            wall;
        inGroups        1(wall);
        nFaces          88392;
        startFace       12144110;
    }
    int-pipe-tube-in-2
    {
        type            wall;
        inGroups        1(wall);
        nFaces          715;
        startFace       12232502;
    }
    int-core-in-1
    {
        type            wall;
        inGroups        1(wall);
        nFaces          11340;
        startFace       12233217;
    }
    wall-core
    {
        type            wall;
        inGroups        1(wall);
        nFaces          1224000;
        startFace       12244557;
    }
    int-core-in-2
    {
        type            wall;
        inGroups        1(wall);
        nFaces          11340;
        startFace       13468557;
    }
    int-core-out-1
    {
        type            wall;
        inGroups        1(wall);
        nFaces          11340;
        startFace       13479897;
    }
    wall-outlet-tank
    {
        type            wall;
        inGroups        1(wall);
        nFaces          88720;
        startFace       13491237;
    }
    int-core-out-2
    {
        type            wall;
        inGroups        1(wall);
        nFaces          11340;
        startFace       13579957;
    }
    int-pipe-tube-out-1
    {
        type            wall;
        inGroups        1(wall);
        nFaces          674;
        startFace       13591297;
    }
    pressure-outlet
    {
        type            patch;
        nFaces          674;
        startFace       13591971;
    }
    wall-outlet-pipe
    {
        type            wall;
        inGroups        1(wall);
        nFaces          4928;
        startFace       13592645;
    }
    int-pipe-tube-out-2
    {
        type            wall;
        inGroups        1(wall);
        nFaces          674;
        startFace       13597573;
    }
)

Thanks again,
Vishsel

[Antimony]

Hi,

mergeMeshes does not create interfaces. That is something that has to be done by the user.

I usually use cyclicAMI to connect two meshes that have been merged. And I do this after I have merged all meshes. You could look around and see what other patchTypes people use for interface.

One other point to note - if I am not wrong, patches with the same name will be merged into one when you use mergeMeshes. So you might want to keep that in mind to ensure that mergeMeshes is not doing something you don't want it to do.

Hope this helps.

Cheers,
Antimony

[Vishsel]

Thankyou so much for your response and feedback.

Best regards,
Vishsel

[Vishsel]

Originally Posted by Antimony

Hi,

mergeMeshes does not create interfaces. That is something that has to be done by the user.

I usually use cyclicAMI to connect two meshes that have been merged. And I do this after I have merged all meshes. You could look around and see what other patchTypes people use for interface.

One other point to note - if I am not wrong, patches with the same name will be merged into one when you use mergeMeshes. So you might want to keep that in mind to ensure that mergeMeshes is not doing something you don't want it to do.

Hope this helps.

Cheers,
Antimony

Hi,

I have done mergeMeshes with same internal patch names and it was merged. Now my question is, how to define a boundary condition for internal patch in U,p,k,T,nut,epsilon dictionary at 0 directory ?


Thanks in advance.

[Vishsel]

11
(
massflow-inlet
{
    type            patch;
    nFaces          715;
    startFace       12137752;
}

wall-inlet-pipe
{
    type            wall;
    inGroups        1 ( wall );
    nFaces          4928;
    startFace       12138467;
}

int-pipe-tube-in
{
    type            patch;
    nFaces          1430;
    startFace       12143395;
}

int-core-in
{
    type            patch;
    nFaces          22680;
    startFace       12144825;
}

wall-inlet-tank
{
    type            wall;
    inGroups        1 ( wall );
    nFaces          88392;
    startFace       12167505;
}

int-core-out
{
    type            patch;
    nFaces          22680;
    startFace       12255897;
}

wall-core
{
    type            wall;
    inGroups        1 ( wall );
    nFaces          1224000;
    startFace       12278577;
}

int-pipe-tube-out
{
    type            patch;
    nFaces          1348;
    startFace       13502577;
}

wall-outlet-tank
{
    type            wall;
    inGroups        1 ( wall );
    nFaces          88720;
    startFace       13503925;
}

pressure-outlet
{
    type            patch;
    nFaces          674;
    startFace       13592645;
}

wall-outlet-pipe
{
    type            wall;
    inGroups        1 ( wall );
    nFaces          4928;
    startFace       13593319;
}

)

Hi all,

This is my boundary file. i have to create boundary condition for internal patches such as
int-pipe-tube-in & out
int-core-in & out
anyone can help me ?

Thankyou in advance.
Vishsel

[Antimony]

Hi,

The patches indicated in the boundary file are technically boundary patches, meaning that you would need to specify BCs on them in the 0 folder for you to start the simulation.

In light of this, I am not sure what exactly you mean...

Cheers,
Antimony

[Vishsel]

Hi Antimony,

That's correct. I am asking how to write a boundary condition for internal patch in U,p,k,T,nut,epsilon dictionary at 0 directory ? like below quotes

Thanks in advance.

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    massflow-inlet
    {
        type            flowRateInletVelocity;
        massFlowRate    constant value;
        value           uniform (0 0 0);
        rho             rho;
        rhoInlet        value;
    }
    pressure-outlet
    {
        type            zeroGradient;
        
    }
    
    wall-inlet-tank
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wall-outlet-tank
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wall-core
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wall-inlet-pipe
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wall-outlet-pipe
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

[Vishsel]

Hi Bruno,

It's possible to do this, but it depends on what exactly you want to do.

For example, there is a tutorial named "TJunctionFan", located in "incompressible/pimpleFoam/TJunctionFan", which creates a cyclic baffle. It then uses a special boundary condition of type "fan"... well, the specifics are in the file "system/createBafflesDict" and in "system/topoSetDict" you can see how the cell faces are selected for later converting to the cyclic baffles.

My case
5 fluid domains = inlet pipe,inlet tank, core,outlet tank,outlet pipe. Between these domains there are internal patches (totally 4 patches). In that patches, I have to monitor the pressure value.

And is it possible to use inletOutlet boundary condition for internal patches? So How to set a boundary conditions for internal patches in U,p,k,T,nut,epsilon dictionary at 0 time folder ?

[wyldckat]

Quick answer: If you study the tutorial case "incompressible/pimpleFoam/RAS/propeller", you should be able to figure out how to make this work in your case: https://github.com/OpenFOAM/OpenFOAM.../RAS/propeller

Steps:

1. You need to edit the file "system/createPatchDict" and inside define the patches you want to connect between regions. For example, you will need something like this:
   

   /*--------------------------------*- C++ -*----------------------------------*\
     =========                 |
     \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
      \\    /   O peration     | Website:  https://openfoam.org
       \\  /    A nd           | Version:  6
        \\/     M anipulation  |
   \*---------------------------------------------------------------------------*/
   FoamFile
   {
       version     2.0;
       format      ascii;
       class       dictionary;
       object      createPatchDict;
   }
   
   // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
   
   // Do a synchronisation of coupled points after creation of any patches.
   // Note: this does not work with points that are on multiple coupled patches
   //       with transformations (i.e. cyclics).
   pointSync false;
   
   // Optional: Write cyclic matches into .obj format; defaults to false.
   writeCyclicMatch  false;
   
   // Patches to create.
   patches
   (
       {
           //- Master side patch
           name            pipeTubeIn;
           patchInfo
           {
               type            cyclicAMI;
               matchTolerance  0.0001;
               neighbourPatch  pipeTubeOut;
               transform       noOrdering;
           }
           constructFrom patches;
           patches (int-pipe-tube-in);
       }
   
       {
           //- Slave side patch
           name            pipeTubeOut;
           patchInfo
           {
               type            cyclicAMI;
               matchTolerance  0.0001;
               neighbourPatch  pipeTubeIn;
               transform       noOrdering;
           }
           constructFrom patches;
           patches (int-pipe-tube-out);
       }
   );
   
   // ************************************************************************* //

2. Notice that I had to change the names of the patches, because OpenFOAM will not create the cyclic patches if the original names are used.
   Just in case you aren't seeing the correspondence between old and new patches:
   • int-pipe-tube-out --> pipeTubeOut
   • int-pipe-tube-in -- > pipeTubeIn
3. Then you need to edit all files you have in the folder "0" and add the new boundary conditions for these new patches, namely:
   

   pipeTubeIn
   {
       type cyclicAMI;
   }
   
   pipeTubeOut
   {
       type cyclicAMI;
   }

4. As for monitoring the flow rates on these patches, you should be able to use the conventional monitoring function objects that are available in OpenFOAM. For example, it's explained here: https://cfd.direct/openfoam/user-gui...31-2480006.2.2

[Vishsel]

Hi Bruno,

Thank you so much for your help. I followed what you have said and the patches were created. This is my createPatchDict file

// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
//       with transformations (i.e. cyclics).
pointSync false;

// Patches to create.
patches
(
    {
        //- Master side patch
        name            pipeTubeIn;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  pipeTubeOut;
            transform       translational;
            separationVector (0 0.64 0)
        }
        constructFrom patches;
        patches (int-pipe-tube-in);
    }

    {
        //- Slave side patch
        name            pipeTubeOut;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  pipeTubeIn;
            transform       translational;
            separationVector (0 -0.64 0)
        }
        constructFrom patches;
        patches (int-pipe-tube-out);
    }
    
    {
        //- Slave side patch
        name            coreIn;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  coreOut;
            transform       translational;
            separationVector (0 0.5 0)
        }
        constructFrom patches;
        patches (int-core-in);
    }
    
    {
        //- Slave side patch
        name            coreOut;
        patchInfo
        {
            type            cyclicAMI;
            matchTolerance  0.0001;
            neighbourPatch  coreIn;
            transform       translational;
            separationVector (0 -0.5 0)
        }
        constructFrom patches;
        patches (int-core-out);
    }
);

// ************************************************************************* //

After decomposePar, i have run the case for porousSimpleFoam as parallel computation. Now i am facing this error.

Create time

Create mesh for time = 0


SIMPLE: no convergence criteria found. Calculations will run for 100 steps.

Reading field p

Reading field U

Reading/calculating face flux field phi

AMI: Creating addressing and weights between 1430 source faces and 1348 target faces
AMI: Patch source sum(weights) min/max/average = 0, 1, 0.621329
AMI: Patch target sum(weights) min/max/average = 0, 1, 0.604025
AMI: Creating addressing and weights between 22680 source faces and 22680 target faces
AMI: Patch source sum(weights) min/max/average = 0, 1, 0.749074
AMI: Patch target sum(weights) min/max/average = 0, 1, 0.749074
Selecting incompressible transport model Newtonian
Selecting RAS turbulence model realizableKE
bounding k, min: 0 max: 1 average: 1
[4] We're sorry, but the application crashed and safe stack tracing isn't available in this current implementation of blueCFD-Core patches for OpenFOAM.

job aborted:
[ranks] message

[0-3] terminated

[4] process exited without calling finalize

[5] terminated

---- error analysis -----

[4] on PC
porousSimpleFoam ended prematurely and may have crashed. exit code 3

---- error analysis -----

Any suggestion ?

Thankyou in advance
Vishsel

[wyldckat]

Quick answers/questions:

1. This:
   

   AMI: Patch source sum(weights) min/max/average = 0, 1, 0.621329

   means that there is an inconsistency in face matching... in other words, there is one or several faces on one patch that do not have any correspondence on the other patch. Therefore if there is no correspondence, then they are technically not connected to each other.
2. The values you defined for the "separationVector" are very concerning, because that means that they are literally 0.5 and 0.64 meters from each other, in each pair. Why?
3. Steps to figure out what's wrong:
   1. Run:
      

      paraFoam

   2. Select in the mesh parts to only show one patch.
   3. Then click on the Apply button.
   4. Choose to show "Surface with edges".
   5. Then menu "File -> Open" and select the same case file again, so that it gets opened twice.
   6. On the second entry, select in the mesh part only the corresponding pair.
   7. Now, apply the filter "Transform" to the second file in the "Pipeline Browser".
   8. Choose to translate the same value you defined in "createPatchDict".
   9. Choose to show "Wireframe".
   10. Now try to see the parts of the mesh that do not match. You need to correct them in the mesher. Any parts that do not match, need to be assigned to another patch that acts as a wall.
   11. Either that, or you need to correct a bit the translation my moving a bit along the other two axis? This is where the "Transform" filter in ParaView can help you.

[Vishsel]

Hi Bruno,

Thanks again. The steps are perfectly works and I got the value of transform.
But actually the Interiors pipeTubeIn and pipeTubeOut translates along x direction (0.144999995827675 0 0) and distance between the coreIn & coreOut interiors are 0.5 meters along y direction, so i have given it as (0 0.5 0).
Q1.)Is it correct?

Q2.)I don't know which transform i have to use for my case, whether noOrdering or translational ?

But i am getting same error while using noOrdering or translational as like below attached code.


And I have shared a case dictionary through private message.

I got this error, after running the command decomposePar

//* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time



Decomposing mesh region0

Create mesh

Calculating distribution of cells
Selecting decompositionMethod scotch

Finished decomposition in 12.87 s

Calculating original mesh data

Distributing cells to processors

Distributing faces to processors

Distributing points to processors

Constructing processor meshes

Processor 0
    Number of cells = 824190
    Number of faces shared with processor 1 = 535
    Number of faces shared with processor 3 = 400
    Number of processor patches = 2
    Number of processor faces = 935
    Number of boundary faces = 341411

Processor 1
    Number of cells = 825225
    Number of faces shared with processor 0 = 535
    Number of faces shared with processor 2 = 690
    Number of processor patches = 2
    Number of processor faces = 1225
    Number of boundary faces = 362705

Processor 2
    Number of cells = 825240
    Number of faces shared with processor 1 = 690
    Number of processor patches = 1
    Number of processor faces = 690
    Number of boundary faces = 362686

Processor 3
    Number of cells = 819554
    Number of faces shared with processor 0 = 400
    Number of faces shared with processor 5 = 2030
    Number of processor patches = 2
    Number of processor faces = 2430
    Number of boundary faces = 226670

Processor 4
    Number of cells = 830681
    Number of faces shared with processor 5 = 1163
    Number of processor patches = 1
    Number of processor faces = 1163
    Number of boundary faces = 83335

Processor 5
    Number of cells = 824966
    Number of faces shared with processor 3 = 2030
    Number of faces shared with processor 4 = 1163
    Number of processor patches = 2
    Number of processor faces = 3193
    Number of boundary faces = 83688

Number of processor faces = 4818
Max number of cells = 830681 (0.691535% above average 824976)
Max number of processor patches = 2 (20% above average 1.66667)
Max number of faces between processors = 3193 (98.8169% above average 1606)

Time = 0
AMI: Creating addressing and weights between 1430 source faces and 1348 target faces
--> FOAM Warning :
    From function AMIMethod<SourcePatch, TargetPatch>::checkPatches()
    in file lnInclude/../AMIInterpolation/AMIInterpolation/AMIMethod/AMIMethod/AMIMethod.C at line 57
    Source and target patch bounding boxes are not similar
    source box span     : (1.00198e-014 0.06985 0.06985)
    target box span     : (2.6007e-014 0.06985 0.06985)
    source box          : (0.145 -0.104925 -0.034925) (0.145 -0.035075 0.034925)
    target box          : (0.145 0.535075 -0.034925) (0.145 0.604925 0.034925)
    inflated target box : (0.140061 0.530136 -0.0398641) (0.149939 0.609864 0.0398641)


--> FOAM FATAL ERROR:
Unable to find initial target face

    From function void Foam::AMIMethod<SourcePatch, TargetPatch>::initialise(label&, label&)
    in file lnInclude/../AMIInterpolation/AMIInterpolation/AMIMethod/AMIMethod/AMIMethod.C at line 139.

FOAM aborting

We're sorry, but the application crashed and safe stack tracing isn't available in this current implementation of blueCFD-Core patches for OpenFOAM.

This application has requested the Runtime to terminate it in an unusual way.
Please contact the application's support team for more information.

Q3.)while running checkMesh, I came to know this. Is this is the problem ?
if this is a problem please help me for further process.
I have used mergeMeshes for merging.

*Number of regions: 40
    The mesh has multiple regions which are not connected by any face.

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           3991103
    faces:            13598247
    internal faces:   12137752
    cells:            4949856
    faces per cell:   5.19934
    boundary patches: 11
    point zones:      0
    face zones:       5
    cell zones:       5

Overall number of cells of each type:
    hexahedra:     2955296
    prisms:        1936
    wedges:        0
    pyramids:      24047
    tet wedges:    0
    tetrahedra:    1968577
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 40
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"
  <<Writing region 0 with 62920 cells to cellSet region0
  <<Writing region 1 with 996230 cells to cellSet region1
  <<Writing region 2 with 78750 cells to cellSet region2
  <<Writing region 3 with 78750 cells to cellSet region3
  <<Writing region 4 with 78750 cells to cellSet region4
  <<Writing region 5 with 78750 cells to cellSet region5
  <<Writing region 6 with 78750 cells to cellSet region6
  <<Writing region 7 with 78750 cells to cellSet region7
  <<Writing region 8 with 78750 cells to cellSet region8
  <<Writing region 9 with 78750 cells to cellSet region9
  <<Writing region 10 with 78750 cells to cellSet region10
  <<Writing region 11 with 78750 cells to cellSet region11
  <<Writing region 12 with 78750 cells to cellSet region12
  <<Writing region 13 with 78750 cells to cellSet region13
  <<Writing region 14 with 78750 cells to cellSet region14
  <<Writing region 15 with 78750 cells to cellSet region15
  <<Writing region 16 with 78750 cells to cellSet region16
  <<Writing region 17 with 78750 cells to cellSet region17
  <<Writing region 18 with 78750 cells to cellSet region18
  <<Writing region 19 with 78750 cells to cellSet region19
  <<Writing region 20 with 78750 cells to cellSet region20
  <<Writing region 21 with 78750 cells to cellSet region21
  <<Writing region 22 with 78750 cells to cellSet region22
  <<Writing region 23 with 78750 cells to cellSet region23
  <<Writing region 24 with 78750 cells to cellSet region24
  <<Writing region 25 with 78750 cells to cellSet region25
  <<Writing region 26 with 78750 cells to cellSet region26
  <<Writing region 27 with 78750 cells to cellSet region27
  <<Writing region 28 with 78750 cells to cellSet region28
  <<Writing region 29 with 78750 cells to cellSet region29
  <<Writing region 30 with 78750 cells to cellSet region30
  <<Writing region 31 with 78750 cells to cellSet region31
  <<Writing region 32 with 78750 cells to cellSet region32
  <<Writing region 33 with 78750 cells to cellSet region33
  <<Writing region 34 with 78750 cells to cellSet region34
  <<Writing region 35 with 78750 cells to cellSet region35
  <<Writing region 36 with 78750 cells to cellSet region36
  <<Writing region 37 with 78750 cells to cellSet region37
  <<Writing region 38 with 996394 cells to cellSet region38
  <<Writing region 39 with 59312 cells to cellSet region39

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology
    massflow-inlet      715      737      ok (non-closed singly connected)
    wall-inlet-pipe     4928     4984     ok (non-closed singly connected)
    pipeTubeIn          1430     1474     ok (non-closed singly connected)
    coreIn              22680    27648    ok (non-closed singly connected)
    wall-inlet-tank     88392    46637    ok (non-closed singly connected)
    coreOut             22680    27648    ok (non-closed singly connected)
    wall-core           1224000  1228896  ok (non-closed singly connected)
    pipeTubeOut         1348     1398     ok (non-closed singly connected)
    wall-outlet-tank    88720    46801    ok (non-closed singly connected)
    pressure-outlet     674      699      ok (non-closed singly connected)
    wall-outlet-pipe    4928     4984     ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-0.0639 -0.104925 -0.237063) (0.49425 0.604925 0.237063)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-2.42398e-016 -2.16456e-015 8.95593e-014) OK.
    Max cell openness = 3.72756e-016 OK.
    Max aspect ratio = 11.0462 OK.
    Minimum face area = 4.53883e-009. Maximum face area = 3.19248e-005.  Face area magnitudes OK.
    Min volume = 1.21833e-013. Max volume = 5.95433e-008.  Total volume = 0.0142551.  Cell volumes OK.
    Mesh non-orthogonality Max: 73.5639 average: 10.0841
   *Number of severely non-orthogonal (> 70 degrees) faces: 1.
    Non-orthogonality check OK.
  <<Writing 1 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 1.10583 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Thanks in advance
Vishsel

[wyldckat]

Quick answers:

Q1) According to the decomposePar, the translation seems to be wrong... namely that it should be the original value you had of "(0 +-0.64 0)" for pipeTubeIn and pipeTubeOut ... and not "(0.14 0 0)"...

Q2) Something weird is going on... the "boundary" file you sent me via PM does not mention the transformation... maybe cyclicAMI does not support transformation? I don't remember ever trying it myself...
edit: It might do the transformation on its own... hence not having a value assigned to it...

And something looks very strange in the output from decomposePar:

    source box span     : (1.00198e-014 0.06985 0.06985)
    target box span     : (2.6007e-014 0.06985 0.06985)
    source box          : (0.145 -0.104925 -0.034925) (0.145 -0.035075 0.034925)
    target box          : (0.145 0.535075 -0.034925) (0.145 0.604925 0.034925)
    inflated target box : (0.140061 0.530136 -0.0398641) (0.149939 0.609864 0.0398641)

The box spans are nearly identical, but it does a crazy inflation from the target box to the expect target box... maybe it's due to the error introduced in the X box spans that don't match?

Which reminds me: in the file "system/controlDict", use the "writeFormat" set to "binary" and not "ascii". You must use this for all mesh operations, including the mergers.


Q3) Uh... 40 regions instead of just 5? I would need to see the exact commands and steps you used to merge the meshes... because this looks like you kept merging meshes several times, instead of just 5?

[Vishsel]

Hi Bruno,

For merging i have used mergeMeshes file1 file2 - both files are folders with 0,constant,system directories & .msh file and i have five domains so i have created 5 file folders with directories & each .msh file for each file folder. (totally five .msh file)

so i have used mergeMeshes command by
mergeMeshes file1 file2 - new 1 time folder are created in file1 folder and i have copied the polymesh file from 1 time folder to constant/polymesh in file1 folder & for each merging like 12 13 14 15 and for each and every mergeMeshes i will copy the polymesh in 1 time folder and paste it in constant/polymesh . and finally i have viewed in paraFoam for conforming the merging of 5 fluid domains and it was merged.

Before merging, i ran fluent3DMeshToFoam abc.msh individually by setting current directory of each file folder for conversion.

For merging the fluid domains, i just given a same name for interiors because patches with the same name will be merged into one when we use mergeMeshes. And patches also created as files i have sent to you.

while exporting from ansys mesh i set it as "ASCII" format and in controlDict file it has "Binary" format.

Thanks in advance
Vishsel.

[wyldckat]

Quick answers:

1. If you use the "-help" argument with OpenFOAM's applications, you will get a bit more information on how to use it, for example:
   

   mergeMeshes -help

2. In order for you to not have to copy the contents of the folder "1" to "constant", you can simply run:
   

   mergeMeshes -overwrite case1 case2

3. If I understood you correctly, you have done something like this:
   

   mergeMeshes -overwrite case1 case2
   mergeMeshes -overwrite case1 case3
   mergeMeshes -overwrite case1 case4
   mergeMeshes -overwrite case1 case5

   If this is essentially what you have been doing, then something is wrong with the original meshes...
4. Within each case folder, before merging the meshes, run this command:
   

   checkMesh -allTopology -allGeometry -constant

   And check if any of them are reporting more than one mesh region.
5. If any of them, before merging, have more than one region, then you need to check what's happening in that mesh.
6. From the output of the checkMesh, confirm that that bounding box of the mesh has the correct values... for example, perhaps one of the meshes was in millimetre and not in metre.

[Vishsel]

Hi Bruno,

Thanks for your support.

Regards,
Vishsel