[samiam1000]

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

[wyldckat]

Greetings Samuele,

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

find $FOAM_TUTORIALS -name createPatchDict
find $FOAM_UTILITIES -name createPatchDict

Best regards,
Bruno

[samiam1000]

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?

[wyldckat]

Originally Posted by samiam1000

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

[mgdenno]

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

[samiam1000]

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

[wyldckat]

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

[ripudaman]

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

Originally Posted by samiam1000

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

[lukasf]

Use the mapFields command:

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.

/*--------------------------------*- 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
(
);

[lukasf]

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.

Originally Posted by lukasf

Use the mapFields command:

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.

/*--------------------------------*- 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
(
);