[CedricVH]

I want to monitor the mass flow rate and the total pressure every iteration at the outlet of my geometry. A good way to do this is using the simpleFunctionObjects (http://openfoamwiki.net/index.php/Co...unctionObjects).

Using simpleFoam, I am able to calculate the mass flow rate, but not the total pressure. My code in the controlDict file is given as:

functions 
(
   massFlow
   {
     type patchMassFlow;
     functionObjectLibs
       (
         "libsimpleFunctionObjects.so"
       );
     verbose true;
     patches
       (
         outlet
       );
   }

   totPress
   {
     type patchAverage;
     functionObjectLibs
       (
         "libsimpleFunctionObjects.so"
       );
     verbose true;
     fields
       (
         ptot
       );
     patches
       (
         outlet
       );
   }
);

The mass flow is reported correctly, but the parameter ptot can not be used, because it has not been calculated by OpenFOAM.

In post-processing, I would first calculate the total pressure with the command "ptot" and then averaging it with the command "patchAverage ptot outlet"

Does anybody know how to implement this using simpleFunctionObjects?

[CedricVH]

Solved: I have modified the simpleFoam solver so that it calculates ptot every iteration.

[farbfilm]

Hi Cedric,

could you please explain me how you modified the solver that it calculates ptot every iteration???

[CedricVH]

I've copied simpleFoam to another directory and renamed all files (mysimpleFoam)

In createFields.H, I changed this:

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

// BEGIN ADD CODE
    Info<< "Reading field ptot\n" <<endl;
    volScalarField ptot
    (
        IOobject
        (
            "ptot",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE           
       ),
       p + 0.5*magSqr(U)
    );
// END ADD CODE

#   include "createPhi.H"

In mysimpleFoam.C, I've added this:

        {
            #include "UEqn.H"
            #include "pEqn.H"
        }

        turbulence->correct();
// BEGIN ADD CODE
        ptot = p + 0.5*magSqr(U);
// END ADD CODE

        runTime.write();

Take care! This formula of ptot is ONLY valid for incompressible cases. I don't know is this is a good way as I have never programmed for OpenFoam, but hey, it works!

[RalphS]

Does anybody know how I can modified the rhoSimpleFoam solver so that it calculates ptot every iteration?

[claco]

Originally Posted by RalphS

Does anybody know how I can modified the rhoSimpleFoam solver so that it calculates ptot every iteration?

Dear RalphS,

Have You heard any more about total pressure calculation in rhoSimpleFoam solver?

Best regards.

Claudio

[RalphS]

Originally Posted by claco

Dear RalphS,

Have You heard any more about total pressure calculation in rhoSimpleFoam solver?

Best regards.

Claudio

Hello Claudio,


I have written a tool, which is able to calculate total pressure.
But i haven't integrated it into the solver. You can use it for post processing.
Are you interesting in this tool? I can also integrate it (after writing some tools and other stuff, i am able to programming on my own) into the solver, but then I need some time.


Regards

Ralph

[claco]

Originally Posted by RalphS

Hello Claudio,


I have written a tool, which is able to calculate total pressure.
But i haven't integrated it into the solver. You can use it for post processing.
Are you interesting in this tool? I can also integrate it (after writing some tools and other stuff, i am able to programming on my own) into the solver, but then I need some time.


Regards

Ralph

Dear Ralph,

can I kindly have this tool in order to integrate it into the solver (by myself)?
Thank You in advance.

Best,

Claudio

[RalphS]

Dear Claudio,

no problem, here is the tool.

my_ptot.C attach

folder Make:

options:

EXE_INC = \
-I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
-I$(LIB_SRC)/turbulenceModels \
-I$(LIB_SRC)/turbulenceModels/compressible/RAS/RASModel \
-I$(LIB_SRC)/finiteVolume/cfdTools \
-I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = \
-lbasicThermophysicalModels \
-lspecie \
-lcompressibleTurbulenceModel \
-lcompressibleRASModels \
-lfiniteVolume \
-lmeshTools


files:

my_ptot.C

EXE = $(FOAM_USER_APPBIN)/my_ptot

[claco]

Originally Posted by RalphS

Dear Claudio,

no problem, here is the tool.

my_ptot.C attach

folder Make:

options:

EXE_INC = \
-I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
-I$(LIB_SRC)/turbulenceModels \
-I$(LIB_SRC)/turbulenceModels/compressible/RAS/RASModel \
-I$(LIB_SRC)/finiteVolume/cfdTools \
-I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = \
-lbasicThermophysicalModels \
-lspecie \
-lcompressibleTurbulenceModel \
-lcompressibleRASModels \
-lfiniteVolume \
-lmeshTools


files:

my_ptot.C

EXE = $(FOAM_USER_APPBIN)/my_ptot

Thank You very much Ralph.
Claudio