CFD Online Discussion Forums - MapFields utility for staggered grid

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - MapFields utility for staggered grid (https://www.cfd-online.com/Forums/openfoam-solving/254108-mapfields-utility-staggered-grid.html)

MapField for different patch and mesh size

Hello all,

I have simulated my case in openfoam with the non staggered mesh. However, I'm going to use mapField utility to map for example velocity field on a rectangular staggered mesh.

How can I do that? Is it possible?!

Thank you in advance.

How did you run an OpenFOAM case with a non-staggered mesh?

Ok, it was my bad explanation.

Let's consider this case in which you've modelled your case with the following mesh:
Attachment 98214

now you are goiing to map the velocity field to the following mesh:
Attachment 98215

The question is how it can be performed?

Try to follow the steps in this post:

https://www.cfd-online.com/Forums/op...tml#post673845

If that does not work for some reason, report the error message here.

Regards

Dear NotOverUnderated,

Thank you for the reply.

I am beginner in mapfield utility, and I need more details in order to handle my case.

Could you provide me some more information regarding the procedures?

Best

I made some progress...

However, I have come across an error about number of target cells:

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/target$ mapFields -consistent -sourceTime 'latestTime' ../source/

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : mapFields -consistent -sourceTime latestTime ../source/

Date   : Jan 20 2024

Time   : 21:54:10

Host   : DESKTOP-TK3D7CI

PID    : 606

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/target

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Source: "/mnt/e/OpenFoam/Run" "source"

Target: "/mnt/e/OpenFoam/Run" "target"



Create databases as time



Source time: 0

Target time: 0.2

Create meshes



Source mesh size: 668000        Target mesh size: 11200







--> FOAM FATAL ERROR: (openfoam-2112 patch=220610)

Incompatible meshes: different number of patches, fromMesh = 7, toMesh = 5



    From Foam::meshToMesh0::meshToMesh0(const Foam::fvMesh&, const Foam::fvMesh&)

    in file meshToMesh0/meshToMesh0.C at line 134.



FOAM exiting

It says that the number of target cells must be greater than the source!

why? It isn't possible to map from fine mesh to course mesh?

Hi Saeed,

as far as I know, mapFields works perfectly fine with mesh with different size. I think the error you're getting is related to the number of patches which is different between the source case and the target case.

I myself used mapFields only in some simple cases. If you're interested to get a quick overview about this utility check this video by József Nagy: https://youtu.be/qUMPdkvKBS8

I can find this thread that I think is related to your case: https://www.cfd-online.com/Forums/op...r-patches.html

I hope this helps.

Regards

NotOverUnderated thanks again.

Yes, it was because of patch issues and I am doing map with different sizes and patches.

However, I tried different commands for executation of mapField;
case 1:

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/Target$ mapFields -consistent -sourceTime 'latestTime' ../source/

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : mapFields -consistent -sourceTime latestTime ../source/

Date   : Jan 21 2024

Time   : 09:50:20

Host   : DESKTOP-TK3D7CI

PID    : 603

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/Target

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Source: "/mnt/e/OpenFoam/Run" "source"

Target: "/mnt/e/OpenFoam/Run" "Target"



Create databases as time



Source time: 0

Target time: 0.2

Create meshes



Source mesh size: 668000        Target mesh size: 11200







--> FOAM FATAL ERROR: (openfoam-2112 patch=220610)

Incompatible meshes: different number of patches, fromMesh = 7, toMesh = 6



    From Foam::meshToMesh0::meshToMesh0(const Foam::fvMesh&, const Foam::fvMesh&)

    in file meshToMesh0/meshToMesh0.C at line 134.



FOAM exiting

case 2:

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/Target$ mapFields -consistent -sourceTime 'latestTime' ../source/ -parallelSource

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : mapFields -consistent -sourceTime latestTime ../source/ -parallelSource

Date   : Jan 21 2024

Time   : 10:01:35

Host   : DESKTOP-TK3D7CI

PID    : 616

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/Target

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Source: "/mnt/e/OpenFoam/Run" "source"

Target: "/mnt/e/OpenFoam/Run" "Target"



Create databases as time

Create target mesh



Target mesh size: 11200



Source processor 0



Source time: 0.2

Target time: 0.2

mesh size: 111513

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch outlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch top has no faces. Not performing mapping for it.



Mapping fields for time 0.2





Source processor 1



Source time: 0.2

Target time: 0.2

mesh size: 111371

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch inlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch outlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch top has no faces. Not performing mapping for it.



Mapping fields for time 0.2





Source processor 2



Source time: 0.2

Target time: 0.2

mesh size: 111116

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch inlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch top has no faces. Not performing mapping for it.



Mapping fields for time 0.2





Source processor 3



Source time: 0.2

Target time: 0.2

mesh size: 111154

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch outlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch bottom has no faces. Not performing mapping for it.



Mapping fields for time 0.2





Source processor 4



Source time: 0.2

Target time: 0.2

mesh size: 111296

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch inlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch outlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch bottom has no faces. Not performing mapping for it.



Mapping fields for time 0.2





Source processor 5



Source time: 0.2

Target time: 0.2

mesh size: 111550

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch inlet has no faces. Not performing mapping for it.

--> FOAM Warning :

    From void Foam::meshToMesh0::calcAddressing()

    in file meshToMesh0/calculateMeshToMesh0Addressing.C at line 148

    Source patch bottom has no faces. Not performing mapping for it.



Mapping fields for time 0.2





End

case 3:

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/Target$ mapFields -sourceTime 'latestTime' ../source/ -parallelSourc

e

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : mapFields -sourceTime latestTime ../source/ -parallelSource

Date   : Jan 21 2024

Time   : 10:10:56

Host   : DESKTOP-TK3D7CI

PID    : 619

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/Target

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Source: "/mnt/e/OpenFoam/Run" "source"

Target: "/mnt/e/OpenFoam/Run" "Target"



Create databases as time

Create target mesh



Target mesh size: 11200



Source processor 0



Source time: 0.2

Target time: 0.2

mesh size: 111513



Mapping fields for time 0.2





Source processor 1



Source time: 0.2

Target time: 0.2

mesh size: 111371



Mapping fields for time 0.2





Source processor 2



Source time: 0.2

Target time: 0.2

mesh size: 111116



Mapping fields for time 0.2





Source processor 3



Source time: 0.2

Target time: 0.2

mesh size: 111154



Mapping fields for time 0.2





Source processor 4



Source time: 0.2

Target time: 0.2

mesh size: 111296



Mapping fields for time 0.2





Source processor 5



Source time: 0.2

Target time: 0.2

mesh size: 111550



Mapping fields for time 0.2





End

The case 3 was performed without any error, but nothing has genereted in latestTime (0.2 second) folder in target!!!

By the way this is my mapFieldDict:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  v2012                                 |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    location    "system";

    object      mapFieldsDict;

}

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



patchMap

(



);



cuttingPatches 

(



);





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

Source blockMesh:

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/source$ checkMesh

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : checkMesh

Date   : Jan 21 2024

Time   : 10:28:06

Host   : DESKTOP-TK3D7CI

PID    : 623

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/source

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Create time



Create mesh for time = 0



Time = 0



Mesh stats

    points:           740740

    faces:            2076200

    internal faces:   1931800

    cells:            668000

    faces per cell:   6

    boundary patches: 7

    point zones:      0

    face zones:       0

    cell zones:       0



Overall number of cells of each type:

    hexahedra:     668000

    prisms:        0

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    0

    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: 1 (OK).



Checking patch topology for multiply connected surfaces...

    Patch               Faces    Points   Surface topology

    inlet               1600     1771     ok (non-closed singly connected)

    outlet              1600     1771     ok (non-closed singly connected)

    cylinder            2400     2640     ok (non-closed singly connected)

    top                 2600     2871     ok (non-closed singly connected)

    bottom              2600     2871     ok (non-closed singly connected)

    back                66800    67340    ok (non-closed singly connected)

    front               66800    67340    ok (non-closed singly connected)



Checking faceZone topology for multiply connected surfaces...

    No faceZones found.



Checking basic cellZone addressing...

    No cellZones found.



Checking geometry...

    Overall domain bounding box (-0.4 -0.4 -0.01) (1 0.4 0.01)

    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)

    Mesh has 3 solution (non-empty) directions (1 1 1)

    Boundary openness (-4.41575e-18 -7.09869e-18 1.66212e-14) OK.

    Max cell openness = 9.0192e-16 OK.

    Max aspect ratio = 65.3413 OK.

    Minimum face area = 1.5997e-08. Maximum face area = 0.000174079.  Face area magnitudes OK.

    Min volume = 3.20006e-11. Max volume = 3.48158e-07.  Total volume = 0.0223749.  Cell volumes OK.

    Mesh non-orthogonality Max: 44.1889 average: 7.86983

    Non-orthogonality check OK.

    Face pyramids OK.

    Max skewness = 0.434082 OK.

    Coupled point location match (average 0) OK.



Mesh OK.



End

Target blockMesh:

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/Target$ blockMesh

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : blockMesh

Date   : Jan 21 2024

Time   : 10:27:14

Host   : DESKTOP-TK3D7CI

PID    : 621

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/Target

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Create time



Creating block mesh from "system/blockMeshDict"

Creating block edges

No non-planar block faces defined

Creating topology blocks



Creating topology patches - from boundary section



Creating block mesh topology



Check topology



        Basic statistics

                Number of internal faces : 0

                Number of boundary faces : 6

                Number of defined boundary faces : 6

                Number of undefined boundary faces : 0

        Checking patch -> block consistency



Creating block offsets

Creating merge list (topological search)...

Deleting polyMesh directory "constant/polyMesh"



Creating polyMesh from blockMesh

Creating patches

Creating cells

Creating points with scale (1 1 1)

    Block 0 cell size :

        i : 0.01 .. 0.01

        j : 0.01 .. 0.01

        k : 0.02 .. 0.02





There are no merge patch pairs



Writing polyMesh with 0 cellZones

----------------

Mesh Information

----------------

  boundingBox: (-0.4 -0.4 -0.01) (1 0.4 0.01)

  nPoints: 22842

  nCells: 11200

  nFaces: 45020

  nInternalFaces: 22180

----------------

Patches

----------------

  patch 0 (start: 22180 size: 80) name: inlet

  patch 1 (start: 22260 size: 80) name: outlet

  patch 2 (start: 22340 size: 140) name: top

  patch 3 (start: 22480 size: 140) name: bottom

  patch 4 (start: 22620 size: 11200) name: front

  patch 5 (start: 33820 size: 11200) name: back



End

Hi again,

I found the problem. The contents of the 0 folder must be inside the latest time (0.2 second) folder.

Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/Target$ mapFields -sourceTime 'latestTime' ../source/ -parallelSource

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2112                                  |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

Build  : _6e1fca0e-20220610 OPENFOAM=2112 patch=220610 version=2112

Arch   : "LSB;label=32;scalar=64"

Exec   : mapFields -sourceTime latestTime ../source/ -parallelSource

Date   : Jan 21 2024

Time   : 11:54:25

Host   : DESKTOP-TK3D7CI

PID    : 762

I/O    : uncollated

Case   : /mnt/e/OpenFoam/Run/Target

nProcs : 1

trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)

allowSystemOperations : Allowing user-supplied system call operations



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

Source: "/mnt/e/OpenFoam/Run" "source"

Target: "/mnt/e/OpenFoam/Run" "Target"



Create databases as time

Create target mesh



Target mesh size: 11200



Source processor 0



Source time: 0.2

Target time: 0.2

mesh size: 111513



Mapping fields for time 0.2



    interpolating nut

    interpolating p

    interpolating k

    interpolating omega

    interpolating U



Source processor 1



Source time: 0.2

Target time: 0.2

mesh size: 111371



Mapping fields for time 0.2



    interpolating nut

    interpolating p

    interpolating k

    interpolating omega

    interpolating U



Source processor 2



Source time: 0.2

Target time: 0.2

mesh size: 111116



Mapping fields for time 0.2



    interpolating nut

    interpolating p

    interpolating k

    interpolating omega

    interpolating U



Source processor 3



Source time: 0.2

Target time: 0.2

mesh size: 111154



Mapping fields for time 0.2



    interpolating nut

    interpolating p

    interpolating k

    interpolating omega

    interpolating U



Source processor 4



Source time: 0.2

Target time: 0.2

mesh size: 111296



Mapping fields for time 0.2



    interpolating nut

    interpolating p

    interpolating k

    interpolating omega

    interpolating U



Source processor 5



Source time: 0.2

Target time: 0.2

mesh size: 111550



Mapping fields for time 0.2



    interpolating nut

    interpolating p

    interpolating k

    interpolating omega

    interpolating U



End

Let's summarize the required steps:

Make Target directory with containing folders of system, constant and latest Time (name it based on the what time step you want, for example here is 0.2 second)
Copy all 0 folder contents (U, P & ...) inside sourse directory to this folder in Target directory
Append MapfieldDict in the system folder in Target
In order to execute mapping go to the target directory and enter the following command (change it based on your case):
Code:

saeedfoam@DESKTOP-TK3D7CI:/mnt/e/OpenFoam/Run/Target$ mapFields -sourceTime 'latestTime' ../source/ -parallelSource

Edit: keep in mind you should execute blockMesh in target directory before running the above command.

That was the case where you can do maping for a specific period of time, now I would like to do maping over runtime through the following utility:

Code:

mapFields1

{

    // Mandatory entries (unmodifiable)

    type            mapFields;

    libs            (fieldFunctionObjects);



    // Mandatory (inherited) entries (runtime modifiable)

    fields          (<field1> <field2> ... <fieldN>);

    mapRegion       coarseMesh;

    mapMethod       cellVolumeWeight;

    consistent      true;



    // Optional entries (runtime modifiable)

    // patchMapMethod  direct;  // AMI-related entry

    // enabled if consistent=false

    // patchMap        (<patchSrc> <patchTgt>);

    // cuttingPatches  (<patchTgt1> <patchTgt2> ... <patchTgtN>);



    // Optional (inherited) entries

    region          region0;

    enabled         true;

    log             true;

    timeStart       0;

    timeEnd         1000;

    executeControl  timeStep;

    executeInterval 1;

    writeControl    timeStep;

    writeInterval   1;

}

So what would be the steps?

I have adopted it inside my controlDict:

Code:

functions

{

     mapFields1

    {

        type            mapFields;

        libs            (fieldFunctionObjects);

        mapRegion       Target;

        mapMethod       cellVolumeWeight;

        consistent      no;

        patchMap        ();

        cuttingPatches  ();

        fields

        (

            U

            p

        );



        executeControl  writeTime;



        writeControl    writeTime;

        

    }



}

Nevertheless, one question left for me about mapRegion Target?!
How can I adopt this part for my case?

Regards

I think you need to create a region. I have never done that myself before but I believe this is easy when checking the cavityMappingTest tutorials.

Code:

$FOAM_TUTORIALS/tutorials/incompressible/icoFoam/cavityMappingTest

In that tutorial only one case is used but two blockMeshDict files are used to create a coarse and a fine meshes.

Code:

# create the coarse mesh

blockMesh -dict system/blockMeshDict.coarse



# move the coarse mesh to its own folder

mv constant/polyMesh constant/coarseMesh



# create the fine mesh

blockMesh -dict system/blockMeshDict.fine

Notice also that there is a folder with the name 'coarseMesh' inside the system directory as well.

Thanks for the information.

Code:

 // Optional (inherited) entries

        region          region0;

It doesn't mandatory to create a region, region0 refers to the entire domain by default and it is optional.

However, in the cavityMappingTest tutorial the mapping over runtime has not mentioned.

I would appreciate any help regarding this matter as well as any idea for mapping all of the time steps with postProcess utility.

Thanks.

In your question you're asking about mapRegion keyword not region keyword.

I am working on it, and it gave me some satisfactory feedback.
Tomorrow I will share my findings.

Best

Dear NotOverUnderated,

I followed the steps of cavityMappingTest, and finally became successful to perform mapping over runTime. However, I have come across another isssue with that.

Original result:Attachment 98238

The interpolated results:Attachment 98239 & Attachment 98240

As you can see, when I use point data illustration, every thing got messed up!

However, mapping of cell data illustration seems good.

Does it depend on the factors of:

Quote:

Options for the mapMethod entry:

direct
mapNearest
cellVolumeWeight
correctedCellVolumeWeight

Options for the patchMapMethod entry:

directAMI
mapNearestAMI
faceAreaWeightAMI
partialFaceAreaWeightAMI

Finally, I found the problem.

The point is I should assign empty type to all patches in the blockMeshDict.course for my case.

Code:

boundary

(

    

    inlet

    {

        type empty;

        faces

        (

            (0 4 7 3)

        );

    }

    outlet

    {

        type empty;

        faces

        (

            (1 5 6 2)

        );

    }

        top

    {

        type empty;

        faces

        (

            (3 2 6 7)

                        

        );

    }

        

        bottom

    {

        type empty;

        faces

        (

            

                        (0 1 5 4)

        );

    }



        front

    {

        type empty;

        faces

        (

                        (0 1 2 3)

                                

        );

    }

        back

    {

        type empty;

        faces

        (

                        

                        (4 5 6 7)        

        );

    }



);

Here is a sample of mapping of flow over a cylinder:

Attachment 98268 & Attachment 98269