CFD Online Discussion Forums - mapField: the same mesh, with one more patch

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

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - mapField: the same mesh, with one more patch (https://www.cfd-online.com/Forums/openfoam/105787-mapfield-same-mesh-one-more-patch.html)

mapField: the same mesh, with one more patch

Dear All,

I am trying to use the mapField command in order to transfer the solution between 2 meshes that are identical.

There is only a difference: in the targetMesh I have added a patch.

How can I solve this?

Thanks a lot,

Samuele

Greetings Samuele,

A quick solution might be to use createPatch on the first case. You can find examples by running:

Code:

find $FOAM_TUTORIALS -name createPatchDict

find $FOAM_UTILITIES -name createPatchDict

Best regards,
Bruno

Hi Bruno and thanks for answering,

actually I thought about creating a patch.

The point is that in case one I have a patch called wall-part_3-solid and I split this patch in two patches for case two: wall-part_3-solid and wall_back.

The point is that I have already the solution for case one.

Is it possible to add a patch on a solved case? Or I should run again the simulation?

Quote:

Originally Posted by samiam1000 (Post 376178)

Is it possible to add a patch on a solved case? Or I should run again the simulation?

I honestly don't know and never tried it on a case that already has a solution... but I think it should work :)
If it doesn't, then it's possibly a bug or missing feature :D

Have you tried using the mapFieldsDict instead of use the -consistent flag?

Dear all,

just one more question.

What can I do if - instead of adding a patch - I'd like to remove a patch?

This is the case: I study a steady solution of a room woth a door.

Suddenly, the door desappears. Hence, I have 2 identical mesh, without the patch ``door''.

I am looking for the removePatch feature. Does this exist?

Thanks a lot,
Samuele

Hi Samuele,

I believe you still have to use createPatch!

But still, you don't need to remove a patch. You can simply define that patch as a wall and set parameters/boundary conditions as if it were a wall!

Best regards,
Bruno

Did you find a solution to this problem?

Samuele,

I have a problem very similar to yours. Were you able to find a solution to the problem you discuss in this thread?

Thank you.
Ripu

Quote:

Originally Posted by samiam1000 (Post 376137)

Use the mapFields command:

Code:

mapFields "pathToSourceCase" -mapMethod mapNearest -targetRegion region0 -sourceTime 'latestTime'

My example:

Source Case: Has a patch called: lowerWall
New Case: Here the patch "lowerWall" is split into: WALL1, WALL2 and lowerWall.

Content of mapFieldsDict.

Code:

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

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

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

|  \\    /   O peration     | Version:  2.1.x                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

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

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    object      mapFieldsDict;

}

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





// List of pairs of source/target patches for mapping

patchMap

(

inlet inlet

outlet outlet

upperWall upperWall

lowerWall WALL1

lowerWall WALL2

lowerWall lowerWall

frontAndBack frontAndBack

);



// List of target patches cutting the source domain (these need to be

// handled specially e.g. interpolated from internal values)

cuttingPatches

(

);

The target case needs a time directory with the correct (empty) fields (boundary conditions and patch-names) prepared.

This way the results from the source file can be interpolated onto the target case.

Quote:

Originally Posted by lukasf (Post 835976)

Use the mapFields command:

Code:

mapFields "pathToSourceCase" -mapMethod mapNearest -targetRegion region0 -sourceTime 'latestTime'

My example:

Source Case: Has a patch called: lowerWall
New Case: Here the patch "lowerWall" is split into: WALL1, WALL2 and lowerWall.

Content of mapFieldsDict.

Code:

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

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

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

|  \\    /   O peration     | Version:  2.1.x                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

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

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    object      mapFieldsDict;

}

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





// List of pairs of source/target patches for mapping

patchMap

(

inlet inlet

outlet outlet

upperWall upperWall

lowerWall WALL1

lowerWall WALL2

lowerWall lowerWall

frontAndBack frontAndBack

);



// List of target patches cutting the source domain (these need to be

// handled specially e.g. interpolated from internal values)

cuttingPatches

(

);