CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Velocity B.C. problem for multiphaseInterFoam

Register Blogs Community New Posts Updated Threads Search

Like Tree1Likes
  • 1 Post By alexeym

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 21, 2019, 13:34
Default Velocity B.C. problem for multiphaseInterFoam
  #1
Member
 
Dokeun, Hwang
Join Date: Apr 2010
Location: Korea, Republic of
Posts: 98
Rep Power: 16
dokeun is on a distinguished road
Hello.

I'm trying to utilizing multiphaseInterFoam for liquid impinging problem.

I got the error message as below
Code:
[3] 
[3] --> FOAM FATAL ERROR: 
[3] 
    request for volVectorField U.air from objectRegistry region0 failed
    available objects of type volVectorField are

3
(
U_0
U
HbyA
)
[3] 
[0] [1] 
[1] 
[1] --> FOAM FATAL ERROR: 
[1] 
    request for volVectorField U.air from objectRegistry region0 failed
    available objects of type volVectorField are

3
(
U_0
U
HbyA
)
[1] 
[1] 
[1]     From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>]
[1]     in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C
[0] 
[0] --> FOAM FATAL ERROR: 
[0] 
    request for volVectorField U.air from objectRegistry region0 failed
    available objects of type volVectorField are

3
(
U_0
U
HbyA
)
[0] 
[0] 
[0]     From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>]
[0]     in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193. at line 193.
[1] 
FOAM parallel run aborting
[1] 
[2] 
[2] 

[0] 
FOAM parallel run aborting
[0] 
[0] #0  Foam::error::printStack(Foam::Ostream&)[2] --> FOAM FATAL ERROR: 
[2] 
    request for volVectorField U.air from objectRegistry region0 failed
    available objects of type volVectorField are

3
(
U_0
U
HbyA
)
[2] 
[2] 
[2]     From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>]
[2]     in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.
[2] 
FOAM parallel run aborting
[2] 
[2] #0  Foam::error::printStack(Foam::Ostream&)[1] #0  Foam::error::printStack(Foam::Ostream&)[3] 
[3]     From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>]
[3]     in file /home/ubuntu/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.
[3] 
FOAM parallel run aborting
[3] 
[3] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[1] #1  Foam::error::abort() at ??:?
[0] #1  Foam::error::abort() at ??:?
[2] #1  Foam::error::abort() at ??:?
[3] #1  Foam::error::abort() at ??:?
[2] #2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
[1] #2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
[3] #2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
[0] #2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
 at ??:?
[2] #3  Foam::totalPressureFvPatchScalarField::updateCoeffs() at ??:?
[3] #3  Foam::totalPressureFvPatchScalarField::updateCoeffs()[1] #3  Foam::totalPressureFvPatchScalarField::updateCoeffs() at ??:?
[0] #3  Foam::totalPressureFvPatchScalarField::updateCoeffs() at ??:?
[1] #4  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
[3] #4  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
[2] #4  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
[0] #4  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
[2] #5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
[1] #5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
[3] #5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
[0] #5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
 at ??:?
[3] #6  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[1] #6  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&)[2] #6  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[0] #6  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
 at ??:?
[1] #7  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&)[2] #7  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[3] #7  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[0] #7  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
[1] #8   at ??:?
[3] #8   at ??:?
[2] #8  ?? at ??:?
[0] #8  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[1] #9   in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[3] #9   in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[2] #9  ???? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[0] #9   in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[1] #10  __libc_start_main in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[2] #10  __libc_start_main in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[3] #10  __libc_start_main? in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #11   in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #11   in "/lib/x86_64-linux-gnu/libc.so.6"
[2] #11  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[0] #10  __libc_start_main?? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/mul in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
tiphaseInterFoam"
 in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
 in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #11  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/multiphaseInterFoam"
[ae118aa2fa16:00524] 3 more processes have sent help message help-mpi-api.txt / mpi-abort
[ae118aa2fa16:00524] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
I don't understand why this error occurs and how to fix it.
I hope someone give me a lesson.
The U.air I have is like
Code:
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U.air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [ 0 1 -1 0 0 0 0 ];

internalField   uniform (0 0 0);

boundaryField
{
    inlet_a
    {
        type            fixedValue;
        value           $internalField;
    }
    wall
    {
        type            noSlip;
    }
    inlet_pph
    {
        type            fixedValue;
        value           $internalField;
    }
    inlet_psh
    {
        type            fixedValue;
        value           $internalField;
    }
    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
  symmetry_l
  {
      type            symmetry;
  }
  symmetry_r
  {
      type            symmetry;
  }
  defaultFaces
  {
      type            empty;
  }
    internalField
    {
        type            fixedValue;
        value           $internalField;
    }
}


// ************************************************************************* //
Sincerely yours.
dokeun is offline   Reply With Quote

Old   April 21, 2019, 16:49
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,930
Rep Power: 38
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

If you look a little bit deeper into error message, you can spot this line:

Code:
Foam::totalPressureFvPatchScalarField::updateCoeffs()
So, the error happes in fact in p_rgh boundary conditions, and U.air file, you have posted, has no value in diagnosing your problem.

If we take a look at totalPressureFvPatchScalarField.C, you will find there this:

Code:
void Foam::totalPressureFvPatchScalarField::updateCoeffs()
{
    updateCoeffs
    (
        p0(),
        patch().lookupPatchField<volVectorField, vector>(UName())
    );
}
So, this method uses UName_ property to look up velocity fields. And in constructor of the boundary field there are these lines:

Code:
Foam::totalPressureFvPatchScalarField::totalPressureFvPatchScalarField
(
    const fvPatch& p,
    const DimensionedField<scalar, volMesh>& iF,
    const dictionary& dict
)
:
    fixedValueFvPatchScalarField(p, iF, dict, false),
    UName_(dict.lookupOrDefault<word>("U", "U")),
...
So, to fix error, you just put "U U.air" into the B.C. dictionary.
dokeun likes this.
alexeym is offline   Reply With Quote

Old   April 21, 2019, 22:23
Thumbs up
  #3
Member
 
Dokeun, Hwang
Join Date: Apr 2010
Location: Korea, Republic of
Posts: 98
Rep Power: 16
dokeun is on a distinguished road
Dear Alexey,
I really appreciate for your instruction.
I found that unnecessary codes were in p_rgh file and delete these lines for U, phi as below.
I won’t solved it without your comment.
Code:
boundaryField
{
   ...
    atmosphere
    {
        type            totalPressure;
        p0              uniform 0;
        //U               U.air;     <- I deleted this line
        //phi             phi.air;  <- I deleted this line
    }
  ....
}
Actually
dokeun is offline   Reply With Quote

Reply

« Previous Thread | Next Thread »

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts
BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
mass inflow B.C. disappears, whereas Velocity inlet B.C. no Ema40 Fluent Multiphase 0 September 16, 2015 10:28
VELOCITY vs VELOCITY IN STN FRAME vs RELATIVE VELOCITY everest20 FLUENT 1 July 13, 2015 08:35
pressure contour and velocity profile problem alee1293 Main CFD Forum 0 July 18, 2014 10:31
Problem with time average tangential velocity in swirl flow. lakhi FLUENT 5 July 18, 2012 16:28
Pressure Velocity coupling problem Sunho park OpenFOAM Running, Solving & CFD 0 August 4, 2010 00:22


All times are GMT -4. The time now is 20:42.

Contact Us - CFD Online - Privacy Statement - Top