Can I get OpenFOAM to Calculate Energy Flux for me?

k13113y · September 13, 2016, 08:21

Hi all,

I'm running a simulation that propagates internal waves through a stratified fluid and I want to calculate the energy flux at various points throughout my domain over time.

The formula for energy flux is simply J = pU and I already have output files for p and U for each time step.

My question is, how do I get OpenFOAM to multiply pressure and velocity and generate a new output file called "energyFlux"?

Thanks

k13113y · September 13, 2016, 08:40

So far I have:

Code:

volVectorField
(
    IOobject
    (
        "energyFlux",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
    ),
    p*U
);

written into the createFields.H file of the interDyMFoam Solver. But I'm unsure of whether this is the right format and how I should recompile the solver.

akidess · September 13, 2016, 09:18

foamCalc multiply p U:
https://openfoamwiki.net/index.php/Contrib_foamCalcEx

g.freeman · September 13, 2016, 09:22

Quote:

Originally Posted by k13113y

So far I have:

Code:

volVectorField
(
    IOobject
    (
        "energyFlux",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
    ),
    p*U
);

written into the createFields.H file of the interDyMFoam Solver. But I'm unsure of whether this is the right format and how I should recompile the solver.

Hello, the correct versione should be like:

Code:

const vector energyFlux = p*U

volVectorField energyFlux
(
    IOobject
    (
        "energyFlux",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    dimensionedScalar("energyFlux",p.dimension*U.dimension,)
);

You need to specify AUTO_WRITE otherwise it will not write anything. You're right when you say to write it into createField.H file; for recompiling the solver just go into the solver folder, in you case $FOAM_SOLVERS/multiphase/interFoam/interDyMFoam, and type wclean, then wmake.

Hope this is useful for you

k13113y · September 13, 2016, 09:24

hey this is great!! Many thanks

My only question now is: does it matter where I place it in the createFields.H file? I'm assuming it must be after p and U...

g.freeman · September 13, 2016, 09:37

Quote:

Originally Posted by k13113y

hey this is great!! Many thanks

My only question now is: does it matter where I place it in the createFields.H file? I'm assuming it must be after p and U...

It doesn't matter since it only reads the fields and then creates the output files.
In the past I've never cared where I write and it has always worked

EDIT: there's a mistake in the last line of the code: after p.dimension()*U.dimension(), after the comma you need to write 0.0.

Code:

dimensionedScalar('energyFlux",p.dimension()*U.dimension(),0.0)

If you prefer you can also specify the dimensions as dimMass/dimTime/dimTime/dimTime, which is pU dimensions.

k13113y · September 13, 2016, 09:45

Hmm I seem to be getting an error when I try to compile.

Code:

Info<< "Reading field energyFlux\n" <<endl;
const vector energyFlux=p_rgh*U;
volVectorField energyFlux
(
    IOobject
    (
        "energyFlux",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
);

Code:

In file included from /opt/openfoam4/src/OpenFOAM/lnInclude/postProcess.H:129:0,
                 from interEnergyFluxFoam.C:58:
./createFields.H: In function ‘int main(int, char**)’:
./createFields.H:32:30: error: conversion from ‘Foam::tmp<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >’ to non-scalar type ‘const vector {aka const Foam::Vector<double>}’ requested
 const vector energyFlux=p_rgh*U;
                              ^
./createFields.H:36:5: error: conflicting declaration ‘Foam::volVectorField energyFlux’
     (
     ^
./createFields.H:32:14: note: previous declaration as ‘const vector energyFlux’
 const vector energyFlux=p_rgh*U;
              ^
./createFields.H:43:42: error: ‘Foam::volScalarField {aka class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                          ^
./createFields.H:43:54: error: ‘Foam::volVectorField {aka class Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                                      ^
./createFields.H:43:22: error: expected primary-expression before ‘(’ token
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                      ^
./createFields.H:43:42: error: ‘Foam::volScalarField {aka class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                          ^
./createFields.H:43:54: error: ‘Foam::volVectorField {aka class Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                                      ^
./createFields.H:43:64: error: expected primary-expression before ‘)’ token
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                                                ^
In file included from interEnergyFluxFoam.C:67:0:
createFields.H:32:30: error: conversion from ‘Foam::tmp<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >’ to non-scalar type ‘const vector {aka const Foam::Vector<double>}’ requested
 const vector energyFlux=p_rgh*U;
                              ^
createFields.H:36:5: error: conflicting declaration ‘Foam::volVectorField energyFlux’
     (
     ^
createFields.H:32:14: note: previous declaration as ‘const vector energyFlux’
 const vector energyFlux=p_rgh*U;
              ^
createFields.H:43:42: error: ‘Foam::volScalarField {aka class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                          ^
createFields.H:43:54: error: ‘Foam::volVectorField {aka class Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                                      ^
createFields.H:43:22: error: expected primary-expression before ‘(’ token
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                      ^
createFields.H:43:42: error: ‘Foam::volScalarField {aka class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                          ^
createFields.H:43:54: error: ‘Foam::volVectorField {aka class Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                                      ^
createFields.H:43:64: error: expected primary-expression before ‘)’ token
     dimensionedScalar("energyFlux",p_rgh.dimension*U.dimension,)
                                                                ^
/opt/openfoam4/wmake/rules/General/transform:8: recipe for target 'Make/linux64GccDPInt32Opt/interEnergyFluxFoam.o' failed
make: *** [Make/linux64GccDPInt32Opt/interEnergyFluxFoam.o] Error 1

I tried removing the dimension and the const variable and the application compiled but the file never appeared in the output.

g.freeman · September 13, 2016, 09:49

I think it is because one argument in dimensionedScalar function is missing, check the edit at my last post

k13113y · September 13, 2016, 09:56

ah sorry, it still has a similar error. I'm using OF 4.0 but I don't think that should matter.

Code:

In file included from /opt/openfoam4/src/OpenFOAM/lnInclude/postProcess.H:129:0,
                 from interEnergyFluxFoam.C:58:
./createFields.H: In function ‘int main(int, char**)’:
./createFields.H:32:30: error: conversion from ‘Foam::tmp<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >’ to non-scalar type ‘const vector {aka const Foam::Vector<double>}’ requested
 const vector energyFlux=p_rgh*U;
                              ^
./createFields.H:36:5: error: conflicting declaration ‘Foam::volVectorField energyFlux’
     (
     ^
./createFields.H:32:14: note: previous declaration as ‘const vector energyFlux’
 const vector energyFlux=p_rgh*U;
              ^
./createFields.H:43:42: error: ‘Foam::volScalarField {aka class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension()*U.dimension(),0.0)
                                          ^
./createFields.H:43:56: error: ‘Foam::volVectorField {aka class Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension()*U.dimension(),0.0)
                                                        ^
In file included from interEnergyFluxFoam.C:67:0:
createFields.H:32:30: error: conversion from ‘Foam::tmp<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >’ to non-scalar type ‘const vector {aka const Foam::Vector<double>}’ requested
 const vector energyFlux=p_rgh*U;
                              ^
createFields.H:36:5: error: conflicting declaration ‘Foam::volVectorField energyFlux’
     (
     ^
createFields.H:32:14: note: previous declaration as ‘const vector energyFlux’
 const vector energyFlux=p_rgh*U;
              ^
createFields.H:43:42: error: ‘Foam::volScalarField {aka class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension()*U.dimension(),0.0)
                                          ^
createFields.H:43:56: error: ‘Foam::volVectorField {aka class Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>}’ has no member named ‘dimension’
     dimensionedScalar("energyFlux",p_rgh.dimension()*U.dimension(),0.0)
                                                        ^
/opt/openfoam4/wmake/rules/General/transform:8: recipe for target 'Make/linux64GccDPInt32Opt/interEnergyFluxFoam.o' failed
make: *** [Make/linux64GccDPInt32Opt/interEnergyFluxFoam.o] Error 1

k13113y · September 13, 2016, 12:15

Okay I have managed to make it work.

Here is what I added to my createFields.H file:

Code:

// Adding a new field: energyFlux

Info<< "Reading field energyFlux\n" <<endl;
volVectorField energyFlux
(
    IOobject
    (
        "energyFlux",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    p_rgh*U
);

and I also made a new file called energyFluxEqn.H inside the interDyMFoam folder (which is the solver I am using). That file is simple and looks like this:

Code:

{
    energyFlux == p_rgh * U;
}

Then I ran:

Code:

wclean
wmake

And now each write interval contains a file called energyFlux.

September 13, 2016, 08:21	Can I get OpenFOAM to Calculate Energy Flux for me?	#1
k13113y New Member Evan Join Date: May 2016 Posts: 23 Rep Power: 9	Hi all, I'm running a simulation that propagates internal waves through a stratified fluid and I want to calculate the energy flux at various points throughout my domain over time. The formula for energy flux is simply J = pU and I already have output files for p and U for each time step. My question is, how do I get OpenFOAM to multiply pressure and velocity and generate a new output file called "energyFlux"? Thanks

September 13, 2016, 08:40		#2
k13113y New Member Evan Join Date: May 2016 Posts: 23 Rep Power: 9	So far I have: Code: volVectorField ( IOobject ( "energyFlux", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), pU ); written into the createFields.H file of the interDyMFoam Solver. But I'm unsure of whether this is the right format and how I should recompile the solver. Last edited by k13113y; September 13, 2016 at 08:41. Reason: code blocks*

September 13, 2016, 09:18		#3
akidess Senior Member Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,377 Rep Power: 29	foamCalc multiply p U: https://openfoamwiki.net/index.php/Contrib_foamCalcEx __________________ On twitter @akidTwit Spend as much time formulating your questions as you expect people to spend on their answer.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
How to calculate the flux of this term grad(alpha1)alphafU?	keepfit	OpenFOAM Running, Solving & CFD	2	June 9, 2016 15:08
How to calculate the flux of this term grad(alpha1)alphafU?	keepfit	OpenFOAM	0	June 6, 2016 10:42
Not able to calculate wall heat flux in cfd post	vikasy123	FLUENT	1	November 21, 2015 00:44
Compare 2D axi-symmetric and 3D. Is OpenFOAM calculate the velocity wrong?	RalphS	OpenFOAM	6	November 13, 2010 20:51
Why FVM for high-Re flows?	Zhong Lei	Main CFD Forum	23	May 14, 1999 13:22

September 13, 2016, 09:24		#5
k13113y New Member Evan Join Date: May 2016 Posts: 23 Rep Power: 9	hey this is great!! Many thanks My only question now is: does it matter where I place it in the createFields.H file? I'm assuming it must be after p and U...

September 13, 2016, 09:49		#8
g.freeman New Member Join Date: May 2016 Posts: 28 Rep Power: 9	I think it is because one argument in dimensionedScalar function is missing, check the edit at my last post

September 13, 2016, 12:15		#10
k13113y New Member Evan Join Date: May 2016 Posts: 23 Rep Power: 9	Okay I have managed to make it work. Here is what I added to my createFields.H file: Code: // Adding a new field: energyFlux Info<< "Reading field energyFlux\n" <<endl; volVectorField energyFlux ( IOobject ( "energyFlux", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), p_rghU ); and I also made a new file called energyFluxEqn.H inside the interDyMFoam folder (which is the solver I am using). That file is simple and looks like this: Code: { energyFlux == p_rgh U; } Then I ran: Code: wclean wmake And now each write interval contains a file called energyFlux.