[mabinty]

Dear all!!

Since a while I ve tried to modify the yPlusRAS utility for a multi region case but haven t succeeded yet. The code compiles but when executed I get the following error message:

Time = 0.001
Reading field p

Reading thermophysical properties

Selecting thermodynamics package hThermo>>>>

Not Implemented
Trying to construct an genericFvPatchField on patch air_to_ceiling of
field h#0 Foam::error:rintStack(Foam:stream&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::genericFvPatchField::genericFvPatchField(Foa m::fvPatch
const&, Foam:imensionedField const&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#3 Foam::fvPatchField::addpatchConstructorToTable >::New(Foam::fvPatch
const&, Foam:imensionedField const&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 Foam::fvPatchField::New(Foam::word const&, Foam::fvPatch const&,
Foam:imensionedField const&) at
~/OpenFOAM/OpenFOAM-1.5.x/src/finiteVolume/lnInclude/newFvPatchField.C:70
#5
Foam::GeometricField::GeometricBoundaryField::Geom etricBoundaryField(Fo am::fvBoundaryMesh const&, Foam:imensionedField const&, Foam::List const&) in "/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#6 Foam::GeometricField::GeometricField(Foam::IOobjec t const&,
Foam::fvMesh const&, Foam::dimensionSet const&, Foam::List const&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#7 Foam::hThermo > > > >::hThermo(Foam::fvMesh const&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#8 Foam::basicThermo::addfvMeshConstructorToTable > > > >
> >::New(Foam::fvMesh const&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#9 Foam::basicThermo::New(Foam::fvMesh const&) in
"/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#10 main at
~/OpenFOAM/aa-1.5.x/applications/yPlusRASCompMultiRegion/yPlusRASCompMultiRegion .C:152
#11 __libc_start_main in "/lib/libc.so.6"
#12 _start in
"/home/aa/OpenFOAM/aa-1.5.x/applications/bin/linux64GccDPOpt/yPlusRASCompMultiRe gion"

>From function genericFvPatchField::genericFvPatchField(const fvPatch&
p, const DimensionedField& iF)
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at
line 45.

FOAM aborting

Aborted

I was searching a bit in the forum and found an entry explaining the error message I received (http://www.cfd-online.com/OpenFOAM_D...ges/1/593.html). So it seems that the solid-fluid interface air_to_ceiling is a default or generic patch field, and hence does not know how to evaluate itself, but what in turn would be necessary to calculated an enthalpy field h (by basicThermo).
When I set disallowGenericFvPatchField to 1 I get the message below:

Create time

Create fluid mesh for region air for time = 0.001

Time = 0.001
Reading field p

Reading thermophysical properties

Selecting thermodynamics package hThermo<pureMixture<constTransport<specieThermo<hC onstThermo<perfectGas>>>>>


Unknown patchField type solidWallMixedTemperatureCoupled for patch type wall

Valid patchField types are :

47
(
fixedGradient
mixedEnthalpy
.
.
etc.
)


file: /home/aa/OpenFOAM/aa-1.5.x/run/chtMultiRegionFoam/hotPlume2D/grid_005/0.001/air/T::air_to_ceiling from line 46 to line 51.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /home/aa/OpenFOAM/OpenFOAM-1.5.x/src/finiteVolume/lnInclude/newFvPatchField.C at line 111.

FOAM exiting

I checked the code of basicThermo.C and saw that there the case of a mixed BC is handled, so I don t know why the solidWallMixedTemperatureCoupled is not allowed.
I would greatly appreciate any comments and advice!!

Thanks in advance,
Aram

[mabinty]

Hi!!

I m about to adapt other utilities like e.g. wallHeatFlux for the multi region case and run always into the same problem. I checked different codes mentioned in the error messages but couldn t find anything out yet; I m stuck now. I kindly ask the community for help, as I strongly depend on these utilities!!!

Thx in advance,
Aram

[gschaider]

Hi Aram!

The Problem is that the boundary condition in question is only known to the cht-Solver. Have a look at the sources of the solver somewhere in $FOAM_SOLVERS/heatTransfer, you will find it there.

The quickest fix might be to add these boundary-conditions to your utility (Add the the C-files to Make/files).

Bernhard

[mabinty]

Hi Bernhard!!

Thank you very much for the great help!! I included the boundary condition as well as the couple manager in the Make/files,options of the utility and it compiles and runs now. I would have two comments:

1.) The first time I ran the utility for a multiRegion case no yPlus was calculated for the new interface air_to_ceiling as its patch type is set to "patch" (I assume by the utility splitMeshRegions) in 0.001/air/polyMesh/boundary. Hence, I changed it to "wall" before exicuting chtMultiRegionFoam and then it worked . I ll try to automatize that. My question now, where else, exept in 0.001/air/polyMesh/boundary are the patch types of boundary faces stored (when I change the patch type after exicuting chtMultiRegionFoam and then run yPlus air_to_ceiling is not recognized as wall)?

2.) Other utilities like e.g. wallHeatFlux would also need the mentioned boundary condition. Is it possible to put them into a library so that all of them have access, or do I have to compile each of the utilities with the BC included in the Make/files,option?

Thx again for the help!! Regards,
Aram

[gschaider]

Originally Posted by mabinty

Hi Bernhard!!

Thank you very much for the great help!! I included the boundary condition as well as the couple manager in the Make/files,options of the utility and it compiles and runs now. I would have two comments:

1.) The first time I ran the utility for a multiRegion case no yPlus was calculated for the new interface air_to_ceiling as its patch type is set to "patch" (I assume by the utility splitMeshRegions) in 0.001/air/polyMesh/boundary. Hence, I changed it to "wall" before exicuting chtMultiRegionFoam and then it worked . I ll try to automatize that. My question now, where else, exept in 0.001/air/polyMesh/boundary are the patch types of boundary faces stored (when I change the patch type after exicuting chtMultiRegionFoam and then run yPlus air_to_ceiling is not recognized as wall)?

I think that the wall-info is only stored in the boundary-file you mentioned. I guess that splitMeshRegions simply can not create walls

Originally Posted by mabinty

2.) Other utilities like e.g. wallHeatFlux would also need the mentioned boundary condition. Is it possible to put them into a library so that all of them have access, or do I have to compile each of the utilities with the BC included in the Make/files,option?

Thx again for the help!! Regards,
Aram

No. You can create a library with the necessary boundary conditions (lets say libchtBCs.so) and then add the line

libs ( "libchtBCs.so");

to the controlDict. Then it is loaded as a "plugin" for every application. Don't know what happens with the solver though (because for that the BCs will be defined twice)

Bernhard

[mabinty]

Hi Bernhard!

Thanks for the fast reply! I ll try the version with the BC in a library and report.

Regards,
Aram

[markusrehm]

Hi Aram,

have you succeeded in creating the library? I am also thinking about how to implement constant heat flux at the walls for a combustion solver.

Regards Markus.

[mabinty]

Dear Markus,

no; honestly I did not try as I had to write new utilities (for yPlus and wallHeatFlux) anyway. So I included the BCs of interest and compiled them together. This works well for me and is doing what I need.
In case you plan to work on such a library I am still interested and would greatly appreciate it if you could share your findings.

All the best,
Aram