CFD Online Discussion Forums - bugs of buoyantBoussinesqPisoFoam or fixedFluxPressure in foam-extend 3.1 and 3.2

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Bugs (https://www.cfd-online.com/Forums/openfoam-bugs/)

- - bugs of buoyantBoussinesqPisoFoam or fixedFluxPressure in foam-extend 3.1 and 3.2 (https://www.cfd-online.com/Forums/openfoam-bugs/172839-bugs-buoyantboussinesqpisofoam-fixedfluxpressure-foam-extend-3-1-3-2-a.html)

bugs of buoyantBoussinesqPisoFoam or fixedFluxPressure in foam-extend 3.1 and 3.2

Dear foamers,
I have found some bugs in foam-extend3.1 and foam-extend3.2
My test case is /heatTransfer/buoyantBoussinesqPisoFoam/hotRoom

[1]bugs in foam-extend 3.1
I changed the pressure boundary from buoyantPressure to fixedFluxPressure,

Quote:

floor
{
type fixedFluxPressure;
rho rhok;
value uniform 0;
adjoint false;
}
ceiling
{
type fixedFluxPressure;
rho rhok;
value uniform 0;
adjoint false;
}
fixedWalls
{
type fixedFluxPressure;
rho rhok;
value uniform 0;
adjoint false;
}

then foam-extend3.1 occurs some errors:

Quote:

Time = 1

Courant Number mean: 0 max: 0 velocity magnitude: 0
DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 8.12238e-06, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for T, Initial residual = 1, Final residual = 2.56071e-06, No Iterations 6

--> FOAM FATAL ERROR:

lookup of (1|A(U)) from objectRegistry region0 successful
but it is not a volScalarField, it is a surfaceScalarField

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/Aaron/foam/foam-extend-3.1/src/foam/lnInclude/objectRegistryTemplates.C at line 120.

FOAM aborting

[2]bugs in foam-extend3.2
then, I run the above case in foam-extend3.2 use one cpu thread, I found it can run!!! and with out "lookup of (1|A(U)) from objectRegistry region0 successful, but it is not a volScalarField, it is a surfaceScalarField" bugs.

However, when I use mpirun, it occurs bugs:

Quote:

Running setHotRoom on /media/Aaron/disk/tutorials_fe31/heatTransfer/buoyantBoussinesqPisoFoam/hotRoom_test
[0] [1]
[1]
[1] --> FOAM FATAL IO ERROR:
[1] wrong token type - expected word found on line 28 the punctuation token '('
[1]
[1] file: /media/Aaron/disk/tutorials_fe31/heatTransfer/buoyantBoussinesqPisoFoam/hotRoom_test/processor1/0/p::boundaryField::floor::rAU at line 28.
[1]
[1] From function operator>>(Istream&, word&)
[1] in file primitives/strings/word/wordIO.C at line 76.
[1]
FOAM parallel run exiting

[0]
[0] --> FOAM FATAL IO ERROR:
[0] wrong token type - expected word found on line 28 the punctuation token '('
[0]
[0] file: /media/Aaron/disk/tutorials_fe31/heatTransfer/buoyantBoussinesqPisoFoam/hotRoom_test/processor0/0/p::boundaryField::floor::rAU at line 28.
[0]
[0] From function operator>>(Istream&, word&)
[0] in file primitives/strings/word/wordIO.C at line 76.
[0] [1]

FOAM parallel run exiting
[0]
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 1 in communicator MPI_COMM_WORLD
with errorcode 1.

Can someone help me solve this bug?

Best Regrads,
Aaron

I am sorry I didn't seen this http://www.cfd-online.com/Forums/ope...d-1-6-ext.html

Quote:

If you have found bugs in the following variants/forks of OpenFOAM:
OpenFOAM 1.6-ext
foam-extend 3.0
foam-extend 3.1
Please report them in the dedicated bug tracker for the Extend Project: http://sourceforge.net/p/openfoam-ex...extendrelease/

how can I delete this post?
or can administrator help me delete this post?

Hi, Foamers
this problem has been solved, check this thread https://sourceforge.net/p/openfoam-e...ndrelease/304/
this is not a bug, change boundary field of p to this, then the case works fine

Quote:

floor
{
type fixedFluxPressure;
rho rhok;
rAU rUA;
}
ceiling
{
type fixedFluxPressure;
rho rhok;
rAU rUA;
}
fixedWalls
{
type fixedFluxPressure;
rho rhok;
rAU rUA;
}

Best,
Aaron

Hi Aaron,

I am using foam extend -3.2 and when i make the changes you suggested in the above posts while using fixedFluxPressure boundary condition, i still get error as shown below. I am using interfoam

Code:



[10] 

[10] 

[10] --> FOAM FATAL ERROR: 

[10]  Field rUA not found for patch groove_1 and field pd

[10] 

[10]     From function void fixedFluxPressureFvPatchScalarField::updateCoeffs()

[10]     in file fields/fvPatchFields/derived/fixedFluxPressure fixedFluxPressureFvPatchScalarField.C at line 168.

[10] 

FOAM parallel run aborting

Code:

  

  groove_1

    {

        type            fixedFluxPressure;

        rho             rho;

        rAU            rUA;



    }

Can you help me in rectifying this ?

Hi, Vignesh

{
type fixedFluxPressure;
rho rhok;
rAU rUA;
}
this change can work in foam-extend-3.1
I encountered the same problem in extend-3.2, so I am not using extend-3.2, sorry I cannot solve your problem......

Hi Aaron,

Thanks for the reply, i found now an intermediate solution.

it works with

{
type fixedFluxPressure;
rho rho;
rAU rAU;
}

After setFields, the last entry changes to (1/A(U)) which must be reset again to rAU. Then the solver runs ... But in parallel, reconstructing the case creates the problem ...