[haewon]

Anybody have parallelize for chtMultiRegionFoam for tutorial in OpenFOAM-1.5.x?
If anyone have an experience, can share your experience?
Thanks.

[nsghaisas]

Hi

I am trying to run the tutorial case multiRegionHeater.tgz provided by Mattijs and the problem I face is that the command splitMeshRegions does not recognize cellZones as an argument.

If I simply run splitMeshRegions without -cellZones, the program says there is only 1 region and dosent do anything,

What could I be doing wrong?

Thanks in advance for any help.

[woody]

Hi Niranjan,

sure you used the command in the right folder??
What is the output of your setsTozones command?

[nsghaisas]

Hi Tobias

The output of setsToZones is givern below.

I am running all commands in the case directory ($FOAM_USR_TUTORIAL/chtMultiRegionFoam/multiRegionHeater)

Thanks
Niranjan


\*---------------------------------------------------------------------------*/
Exec : setsToZones -noFlipMap
Date : Nov 17 2008
Time : 04:51:26
Host : localhost.localdomain
PID : 19964
Case : /home/niranjan/OpenFOAM/OpenFOAM-1.5/tutorials/chtMultiRegionFoam/multiRegionHea ter
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Seached : "constant/polyMesh/sets"
Found :
5
(
topAir
heater
bottomAir
rightSolid
leftSolid
)


pointSets:
0
(
)

cellSets:
5
(
heater
topAir
leftSolid
bottomAir
rightSolid
)

faceSets:
0
(
)

Writing mesh.

End

[woody]

Hi Niranjan,

My output is after cellSets:

Adding set heater as a cellZone.
Adding set topAir as a cellZone.
Adding set leftSolid as a cellZone.
Adding set bottomAir as a cellZone.
Adding set rightSolid as a cellZone.

so there seems to be an error before... did you manipulate the cell regions??

Did your setSet run well (any region sets w/o cells)?

[mahendra]

hi Niranjan..

Do u have the ChtMultiRegionFoam tutorial? I was unable to download it. If you have can you please send it to me at mahendra.wankhede@gmail.com

Where in Pune do you reside and what do you do?

Regards,
Mahendra

[nsghaisas]

Tobias,

I executed the script Allrun as it is and I faced this problem. The log files generated are given below.

From log.setSet, you can see that there is no error. But it does not give the output you've mentioned either.

I havent changed anything manually. I did try to open files in constant/ and constant/polyMesh/sets directories to try to make some sense, but I havent modified anything.

Thanks and regards
Niranjan



log.blockMesh
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : blockMesh
Date : Nov 17 2008
Time : 06:10:31
Host : localhost.localdomain
PID : 20959
Case : /home/niranjan/OpenFOAM/niranjan-1.5/tutorials/multiRegionHeater
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time


Reading block mesh description dictionary

Creating block mesh

Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty

Check block mesh topology

Basic statistics
Number of internal faces : 0
Number of boundary faces : 6
Number of defined boundary faces : 6
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Writing polyMesh

end



log.setSet

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : setSet -batch makeCellSets.setSet
Date : Nov 17 2008
Time : 06:10:32
Host : localhost.localdomain
PID : 20960
Case : /home/niranjan/OpenFOAM/niranjan-1.5/tutorials/multiRegionHeater
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time:0 cells:3000 faces:9700 points:3751 patches:6
Reading commands from file "makeCellSets.setSet"
Please type 'help', 'quit' or a set command after prompt.
Doing:"cellSet heater new boxToCell (-0.01 0 -100 )(0.01 0.01 100)"
Set:heater Size:0 Action:new
Adding cells with center within box (-0.01 0 -100) (0.01 0.01 100)
Writing heater (size 40) to "constant/polyMesh/sets/heater" and to vtk file "VTK/heater/heater_1.vtk"

Doing:"cellSet heater add boxToCell (-0.01 -100 -0.01)(0.01 0.01 0.01)"
Set:heater Size:40 Action:add
Backing up heater into heater_old
Adding cells with center within box (-0.01 -100 -0.01) (0.01 0.01 0.01)
Writing heater (size 80) to "constant/polyMesh/sets/heater" and to vtk file "VTK/heater/heater_1.vtk"

Doing:"cellSet leftSolid new boxToCell (-100 0 -100 )(-0.01 0.01 100)"
Set:leftSolid Size:0 Action:new
Adding cells with center within box (-100 0 -100) (-0.01 0.01 100)
Writing leftSolid (size 130) to "constant/polyMesh/sets/leftSolid" and to vtk file "VTK/leftSolid/leftSolid_1.vtk"

Doing:"cellSet rightSolid new boxToCell (0.01 0 -100 )(100 0.01 100)"
Set:rightSolid Size:0 Action:new
Adding cells with center within box (0.01 0 -100) (100 0.01 100)
Writing rightSolid (size 130) to "constant/polyMesh/sets/rightSolid" and to vtk file "VTK/rightSolid/rightSolid_1.vtk"

Doing:"cellSet topAir new boxToCell (-100 0.01 -100 )(100 100 100)"
Set:topAir Size:0 Action:new
Adding cells with center within box (-100 0.01 -100) (100 100 100)
Writing topAir (size 1200) to "constant/polyMesh/sets/topAir" and to vtk file "VTK/topAir/topAir_1.vtk"

Doing:"cellSet bottomAir clear"
Set:bottomAir Size:0 Action:clear
Writing bottomAir (size 0) to "constant/polyMesh/sets/bottomAir" and to vtk file "VTK/bottomAir/bottomAir_1.vtk"

Doing:"cellSet bottomAir add cellToCell heater"
Set:bottomAir Size:0 Action:add
Adding all elements of cellSet heater ...
Writing bottomAir (size 80) to "constant/polyMesh/sets/bottomAir" and to vtk file "VTK/bottomAir/bottomAir_1.vtk"

Doing:"cellSet bottomAir add cellToCell leftSolid"
Set:bottomAir Size:80 Action:add
Backing up bottomAir into bottomAir_old
Adding all elements of cellSet leftSolid ...
Writing bottomAir (size 210) to "constant/polyMesh/sets/bottomAir" and to vtk file "VTK/bottomAir/bottomAir_1.vtk"

Doing:"cellSet bottomAir add cellToCell rightSolid"
Set:bottomAir Size:210 Action:add
Backing up bottomAir into bottomAir_old
Adding all elements of cellSet rightSolid ...
Writing bottomAir (size 340) to "constant/polyMesh/sets/bottomAir" and to vtk file "VTK/bottomAir/bottomAir_1.vtk"

Doing:"cellSet bottomAir add cellToCell topAir"
Set:bottomAir Size:340 Action:add
Backing up bottomAir into bottomAir_old
Adding all elements of cellSet topAir ...
Writing bottomAir (size 1540) to "constant/polyMesh/sets/bottomAir" and to vtk file "VTK/bottomAir/bottomAir_1.vtk"

Doing:"cellSet bottomAir invert"
Set:bottomAir Size:1540 Action:invert
Backing up bottomAir into bottomAir_old
Writing bottomAir (size 1460) to "constant/polyMesh/sets/bottomAir" and to vtk file "VTK/bottomAir/bottomAir_1.vtk"

End of batch file

End




log.setsToZones

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : setsToZones -noFlipMap
Date : Nov 17 2008
Time : 06:10:32
Host : localhost.localdomain
PID : 20962
Case : /home/niranjan/OpenFOAM/niranjan-1.5/tutorials/multiRegionHeater
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Seached : "constant/polyMesh/sets"
Found :
5
(
topAir
heater
bottomAir
rightSolid
leftSolid
)


pointSets:
0
(
)

cellSets:
5
(
heater
topAir
leftSolid
bottomAir
rightSolid
)

faceSets:
0
(
)

Writing mesh.

End


log.splitMeshRegions

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Usage: splitMeshRegions [-insidePoint point] [-case dir] [-parallel] [-largestOnly] [-help] [-doc] [-srcDoc]


Invalid option: -cellZones


FOAM exiting

[woody]

Dear Niranjan,

my output looks quite different. Typing splitMeshRegions -help I get some output like this:
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Usage: splitMeshRegions [-cellZones] [-blockedFaces faceSet] [-overwrite] [-insidePoint point] [-case dir] [-parallel] [-largestOnly] [-makeCellZones] [-help] [-doc] [-srcDoc]

and the splitting works very well. Are you sure, you installed OF properly?

Regards Tobias

[mahendra]

Dear All,

The case multiRegionHeater ran sucessfully when i executed the commands one by one.

And when I exported the mesh and result files to fluent, using "foamMeshToFluent" and foamDataToFluent" I got nothing to see. Also the mesh file shows only minimum and maximum boundaries and no split regions.

Can anyone guide me to the problem and it's resolution.

Thanks and Regards,
Mahendra

[nsghaisas]

Hi Tobias.

There was some problem with my installation. The case ran successfully when I tried it on a different machine. Thanks for your help.

Mahendra, the answer to your question is there in this thread itself in a post by Andrea.

Niranjan

[mahendra]

hi Niranjan...

I was asking for viewing the results and mesh from OpenFOAM into Fluent.

Mahendra.

[mattijs]

The cht solver uses multiple 'regions'. These get stored as separate subdirectories inside the time directories. Compare the time directories to those of e.g. the cavity tutorial.

Some postprocess tools have a '-region' option to specify which region to work on (e.g. foamToVTK). I don't think foamMeshToXXX has such an option so you'll have to copy the mesh and data (of the region you want to look at) to a separate case. See also http://openfoamwiki.net/index.php/Ho...rocMultiregion.

[nsghaisas]

Mahendra,


An oversight... sorry

[woody]

Hi,

i managed refining a part of the tutorial grid. I just did some manipulations:
adding two files called "cellSetDict.1" and "refineMeshDict" in the system directory.
"cellSetDict.1" should look like this:

-------------------------------------------------------------------------------- --------------------

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object cellSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
name c0;
action new;
topoSetSources
(
boxToCell
{
box (0.01 -100 -0.02)(0.02 0 0.02);
}
);
// ************************************************** *********************** //
-------------------------------------------------------------------------------- --------------------

The refineMeshDict" file looks like this:

-------------------------------------------------------------------------------- --------------------

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*------------------------------------------------------------------------------ -------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object refineMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
set c0;
coordinateSystem global;
globalCoeffs
{
tan1 (1 0 0);
tan2 (0 1 0);
}
directions
(
tan1
tan2
normal
);
useHexTopology yes;
geometricCut no;
writeMesh no;
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

-------------------------------------------------------------------------------- --------------------

Second, I manipulated Allun:

-------------------------------------------------------------------------------- ----
#* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *#
#!/bin/sh
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions

refineMeshByCellSet()
{
echo "creating cell set for primary zone - $1"
cp system/cellSetDict.$1 system/cellSetDict
cellSet >& log.cellSet.$1

echo "refining primary zone - $1"
refineMesh -dict -overwrite >& log.refineMesh.$1
rm constant/polyMesh/sets/*_old
}
rm -r constant/polyMesh/sets
runApplication blockMesh
runApplication setSet -batch makeCellSets.setSet
rm constant/polyMesh/sets/*_old
runApplication setsToZones -noFlipMap
refineMeshByCellSet 1
runApplication splitMeshRegions -cellZones
changeDictionary -region bottomAir
changeDictionary -region topAir
changeDictionary -region heater
changeDictionary -region leftSolid
changeDictionary -region rightSolid
runApplication chtMultiRegionFoam

cp -r 0.001/bottomAir/polyMesh/ constant/bottomAir/.
cp -r 0.001/topAir/polyMesh/ constant/topAir/.
cp -r 0.001/heater/polyMesh/ constant/heater/.
cp -r 0.001/leftSolid/polyMesh/ constant/leftSolid/.
cp -r 0.001/rightSolid/polyMesh/ constant/rightSolid/.
foamToVTK -region bottomAir
foamToVTK -region topAir
foamToVTK -region heater
foamToVTK -region leftSolid
foamToVTK -region rightSolid
#* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *#

-------------------------------------------------------------------------------- --------------------

and Allclean:

-------------------------------------------------------------------------------- --------------------

#* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *#
#!/bin/sh
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions

rm -r VTK
rm -rf constant/polyMesh/sets > /dev/null 2>&1
rm -rf 0/polyMesh > /dev/null 2>&1
rm system/cellSetDict > /dev/null 2>&1
cleanCase
#* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *#

-------------------------------------------------------------------------------- --------------------

,that's it. Hope this helps.

Tobias

[woody]

Hello,

there is one thing coming up in my simulation?

Is it possible to change the patch type for the Interface patch to wall directly??

I need this because otherwise, my turbulent wallfunctions won't be computed, will they?

Which polyMesh/boundary file will be looked up and compared to??

Thanks Tobias

[yibingxin]

Hi,

I got an error when trying the Allrun with the tutorial case. All suggestions/comments are appreciated. Thanks.

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : chtMultiRegionFoam
Date : Dec 03 2008
Time : 08:57:30
Host : FMCompute04
PID : 25608
Case : /nfshome/xiny/OpenFOAM/OpenFOAM-1.5/tutorials/chtMultiRegionFoam/multiRegionHeat er
nProcs : 1

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create fluid mesh for region bottomAir for time = 0.001

Create fluid mesh for region topAir for time = 0.001

Create solid mesh for region heater for time = 0.001

Create solid mesh for region leftSolid for time = 0.001
Create solid mesh for region rightSolid for time = 0.001

*** Reading fluid mesh thermophysical properties for region bottomAir

Adding to pdf

Adding to thermof

Selecting thermodynamics package hThermo<puremixture<consttransport<speciethermo<hc onstthermo<perfectgas>>>>>
Adding to rhof

Adding to Kf



Not implemented#0 Foam::error::printStack(Foam:stream&) in "/nfshome/xiny/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/nfshome/xiny/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::basicThermo::e() const in "/nfshome/xiny/OpenFOAM/OpenFOAM-1.5/lib/linux64GccDPOpt/libbasicThermophysicalM odels.so"
#3 main in "/nfshome/xiny/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/chtMultiRe gionFoam"
#4 __libc_start_main in "/lib64/tls/libc.so.6"
#5 Foam::regIOobject::readIfModified() in "/nfshome/xiny/OpenFOAM/OpenFOAM-1.5/applications/bin/linux64GccDPOpt/chtMultiRe gionFoam"



From function basicThermo::e()
in file basicThermo/basicThermo.H at line 194.

FOAM aborting (FOAM_ABORT set)

[nandiganavishal]

Hi All,

I am new to Openfoam. I just downloaded the tutorial and would like to know where is the solidwallHeatflux boundary condition used in the tutorial. Can anyone help me out in explaining this. Because I have a case where I need to set B.cs given by the equation

-D1*dC1/dn - K1*C1*dPhi/dn = 0 where n is the normal direction.
I am solving a 2d system hence I want to set the flux in the y direction as zero. i.e
-D1*dC1/dy - K1*C1*dPhi/dy = 0
where C1 and Phi are my variables.

Can anyone suggest how exactly I have to go about incorporating this boundary condition.

Thanks

Regards

Vishal

[mabinty]

Dear all!!

I would like to adapt yPlusRAS utility to calculated/written y+ only in the fluid region. I already managed (at least I believe so) to adapt yPlusRAS for a compressible case (yPLusRASCompressible). I tried to realize that yPLusRASCompressible follows the structure of the
time directories "timeName/fluidRegionName" (e.g. 51/topAir) to access
the needed fields for the calculation of yPlus in the fluidRegionName region. The problem occures when creating the "phi" field like:

surfaceScalarField phi
(
IOobject
(
"phi",
runTime.timeName(),
fluidRegions[i],
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
linearInterpolate(rho[i]*U[i])
& fluidRegions[i].Sf()
);

I get the following error message from the compiler:

yPlusRASCompMultiRegion.C: In function 'int main(int, char**)': yPlusRASCompMultiRegion.C:176: error: no matching function for call to 'linearInterpolate(Foam::Vector<double>)'

I wounder because the linearInterpolate-function should be available as included by -I$(LIB_SRC)/finiteVolume/lnInclude. I would greatly appreciate any hint on that! Thx in advance,

Aram

[mabinty]

Dear all!!

I would like to adapt yPlusRAS utility to calculated/written y+ only in the fluid region. I already managed (at least I believe so) to adapt yPlusRAS for a compressible case (yPLusRASCompressible). I tried to realize that yPLusRASCompressible follows the structure of the
time directories "timeName/fluidRegionName" (e.g. 51/topAir) to access
the needed fields for the calculation of yPlus in the fluidRegionName region. The problem occures when creating the "phi" field like:

surfaceScalarField phi
(
IOobject
(
"phi",
runTime.timeName(),
fluidRegions[i],
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
linearInterpolate(rho[i]*U[i])
& fluidRegions[i].Sf()
);

I get the following error message from the compiler:

yPlusRASCompMultiRegion.C: In function 'int main(int, char**)': yPlusRASCompMultiRegion.C:176: error: no matching function for call to 'linearInterpolate(Foam::Vector<double>)'

I wounder because the linearInterpolate-function should be available as included by -I$(LIB_SRC)/finiteVolume/lnInclude. I would greatly appreciate any hint on that! Thx in advance,

Aram

[mabinty]

Hi!!

The code compiles now after removing the indix [i] at rho and U to compute the phi field. But when executing the yPlusRASCompMultiRegion I get the error message shown below at the point where thermophysical properties are read:

Time = 1.001
Reading field p

Reading thermophysical properties

Selecting thermodynamics package hThermo<puremixture<consttransport<speciethermo<hc onstthermo<perfectgas>>>>>


Not Implemented
Trying to construct an genericFvPatchField on patch air_to_ceiling of field h#0 Foam::error::printStack(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<double>::genericFvPatchF ield(Foam::fvPatch const&, Foam::DimensionedField<double,> const&) in "/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#3 Foam::fvPatchField<double>::addpatchConstructorToT able<foam::genericfvpatchfield <double> >::New(Foam::fvPatch const&, Foam::DimensionedField<double,> const&) in "/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 Foam::fvPatchField<double>::New(Foam::word const&, Foam::fvPatch const&, Foam::DimensionedField<double,> const&) at ~/OpenFOAM/OpenFOAM-1.5.x/src/finiteVolume/lnInclude/newFvPatchField.C:70
#5 Foam::GeometricField<double,>::GeometricBoundaryFi eld::GeometricBoundaryField(Fo am::fvBoundaryMesh const&, Foam::DimensionedField<double,> const&, Foam::List<foam::word> const&) in "/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#6 Foam::GeometricField<double,>::GeometricField(Foam ::IOobject const&, Foam::fvMesh const&, Foam::dimensionSet const&, Foam::List<foam::word> const&) in "/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#7 Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hc onstthermo<foam::perfectgas> > > > >::hThermo(Foam::fvMesh const&) in "/home/aa/OpenFOAM/OpenFOAM-1.5.x/lib/linux64GccDPOpt/libbasicThermophysicalMode ls.so"
#8 Foam::basicThermo::addfvMeshConstructorToTable<foa m::hthermo<foam::puremixture<f oam::consttransport<foam::speciethermo<foam::hcons tthermo<foam::perfectgas> > > > > >::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<type>::genericFvPatchField(con st fvPatch& p, const DimensionedField<type,>& iF)
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 45.

FOAM aborting

Aborted

I dug a bit in genericFvPatchField.C and basicThermo.C/.H but couldn t figure out yet what the error message tries to tell me. Could anybody give me a suggestion please!!

Thx in advance!
Aram