|
[Sponsors] |
August 9, 2012, 03:15 |
mapField: the same mesh, with one more patch
|
#1 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 18 |
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 |
|
August 9, 2012, 06:24 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
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 Bruno
__________________
|
|
August 9, 2012, 06:31 |
|
#3 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 18 |
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? |
|
August 9, 2012, 06:33 |
|
#4 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
Quote:
If it doesn't, then it's possibly a bug or missing feature
__________________
|
||
August 10, 2012, 20:59 |
|
#5 |
Senior Member
Matthew Denno
Join Date: Feb 2010
Posts: 138
Rep Power: 16 |
Have you tried using the mapFieldsDict instead of use the -consistent flag?
|
|
October 29, 2012, 05:36 |
|
#6 |
Senior Member
Samuele Z
Join Date: Oct 2009
Location: Mozzate - Co - Italy
Posts: 520
Rep Power: 18 |
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 |
|
October 31, 2012, 13:29 |
|
#7 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128 |
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
__________________
|
|
January 8, 2014, 19:01 |
Did you find a solution to this problem?
|
#8 |
Member
Ripudaman Manchanda
Join Date: May 2013
Posts: 55
Rep Power: 12 |
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 |
|
September 16, 2022, 09:11 |
|
#9 |
Senior Member
Lukas Fischer
Join Date: May 2018
Location: Germany, Munich
Posts: 117
Rep Power: 7 |
Use the mapFields command:
Code:
mapFields "pathToSourceCase" -mapMethod mapNearest -targetRegion region0 -sourceTime 'latestTime' 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 ( ); |
|
January 19, 2023, 02:44 |
|
#10 | |
Senior Member
Lukas Fischer
Join Date: May 2018
Location: Germany, Munich
Posts: 117
Rep Power: 7 |
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:
|
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[snappyHexMesh] SnappyHexMesh for internal Flow | vishwa | OpenFOAM Meshing & Mesh Conversion | 24 | June 27, 2016 08:54 |
[snappyHexMesh] No layers in a small gap | bobburnquist | OpenFOAM Meshing & Mesh Conversion | 6 | August 26, 2015 09:38 |
Create a GeometricField of a given type on given patch? | philippose | OpenFOAM Programming & Development | 4 | August 12, 2013 12:41 |
3D Hybrid Mesh Errors | DarrenC | ANSYS Meshing & Geometry | 11 | August 5, 2013 06:42 |
chtMultiRegionFoam Tutorial | m.nichols19 | OpenFOAM | 12 | September 9, 2010 11:56 |