[MaxxiKing]

Hello everyone,

I try to map the fields from a chtMultiRegionSimpleFoam case to a new chtMultiRegionSimpleFoam case with other boundary conditions.

Therefore I run the command:

mapFields {source_workdir} -case {workdir} -sourceTime '{latest_time}' -sourceRegion {source_region} -targetRegion {target_region} -consistent

But after running mapFields, the boundary conditions in the {workdir} are overwritten by the boundary conditions of the {source_workdir}.

I have tried to map only the internalField with the help of this post (using a mapFieldsDict with empty patchMap and cuttingPatches), but the boundary conditions are still overwritten.

Does anyone know how to map only the internalFields?

Thank you very much!

I am using openFoam Version 2206

[MaxxiKing]

I found a solution:

1. map the fields
2. convert each region from binary to ascii with
   

   foamDictionary {case_dir}/system/controlDict -entry writeFormat -set ascii
   foamFormatConvert -region {region}

3. update the boundary conditions with foamDictionary with e.g.:

   'foamDictionary {case_dir}/0/{region}/T -entry "boundaryField/{patch}/h" -set "uniform 25.0"'

   to set h in externalWallHeatFluxTemperature:
   
   

   boundaryField
   {
       a4ee84fced4c0414bbd71e87bf9631bc6
       {
           type            externalWallHeatFluxTemperature;
           mode            coefficient;
           Ta              uniform 268.15;
           h               uniform 25;
           kappaMethod     solidThermo;
           value           nonuniform List<scalar> 
           132
           (
           268.306
           ...
           )
           ;
      }

4. convert from ascii to binary with
   
   

   foamDictionary {case_dir}/system/controlDict -entry writeFormat -set binary
   foamFormatConvert -region {region}

[fconcli]

To avoid to map the fields you need a mapFieldsDict with an empty field "patchMap"... moreover, remove the "consistent" option when mapping.