[maysmech]

Hi,

I need DU/Dt values for all grids.

How can i calculate and write this parameter.

Any suggestion will be appreciated.

[nimasam]

look in UEqn, something like
volVectorField DuDt= fvc::ddt(U) +fvc::div(phi,U)

[maysmech]

Thanks Nima,

When i switch from Euler to CrancNicholson in fvScheme, ddt0(U) and ddt0(phi) are Written in time folders.

Now, my questions are:

1- is this value equal to D/DT(U)? if no How it can be calculated.

2- Is it any way to write it with Euler ddt scheme?

Regards.

[alberto]

Here it is:

DDtU =
          fvc::ddt(U)
  + fvc::div(phi, U)
  - fvc::div(phi)*U;

To write the field, simply declare it with the appropriate IOobject.

Best,

[maysmech]

Dear Alberto,
Thanks for your answer.
Is it possible to describe more.
Where should i write this code?
What is steps for writing process in time folders?
Is it need to define DDT in folder 0?
I am running LES with pisoFoam.
Regards.

[alberto]

Originally Posted by maysmech

Dear Alberto,
Thanks for your answer.
Is it possible to describe more.
Where should i write this code?
What is steps for writing process in time folders?
Is it need to define DDT in folder 0?
I am running LES with pisoFoam.
Regards.

This questions sounds a bit like "please do my homework", since this stuff is standard.

Take a look at createFields.H, where other fields are created, and do something similar for DDtU. Then update the field at the end of the iteration, before runTime.write().

You do not need to do anything in 0 if you specify NO_READ in the IOobject.

Best,

[maysmech]

Originally Posted by alberto

This questions sounds a bit like "please do my homework", since this stuff is standard.

Take a look at createFields.H, where other fields are created, and do something similar for DDtU. Then update the field at the end of the iteration, before runTime.write().

You do not need to do anything in 0 if you specify NO_READ in the IOobject.

Best,

Thanks
it is my first openFoam programming and it was the cause of my silly questions.
Now i have a scientific question. first i describe my works:

1- Copying pisoFoam to new folder pisoFoam2.

2-Adding below code next of U and P IOobject of creatFields.H:

    volVectorField DDtU
    (
        IOobject
        (
            "DDtU",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

3-Adding below code to before of runTime.write(); of pisoFoam.C:

    DDtU =
               fvc::ddt(U)
             + fvc::div(phi, U)
         - fvc::div(phi)*U;

4- Changing pisoFoam2/Make/files with:

EXE = $(FOAM_APPBIN)/pisoFoam2

5-wmake.

After this steps and running a case with pisoFoam2 this error is displayed:

Reading field p

Reading field U



--> FOAM FATAL ERROR: 
NO_READ specified for read-constructor of object DDtU of class IOobject

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 46.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  Foam::regIOobject::readStream() in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#3  Foam::regIOobject::readStream(Foam::word const&) in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#4  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&) in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/pisoFoam2"
#5  
 in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/pisoFoam2"
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  
 in "/home/maysam/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/pisoFoam2"
Aborted

Switching NO-READ to MUST-READ and defining DDtU in 0 folder solves this error but the problem is i don't know boundary values for this variable.

Regards.

[gregor]

sorry double post

[gregor]

hi its because you are using the wrong constructor

look for example at the createfields.H from the coalChemistryFoam Solver

    DimensionedField<scalar, volMesh> kappa
    (
        IOobject
        (
            "kappa",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimless, 0.0)
    );

there dimensionedScalar("zero", dimless, 0.0) is the value you prescribe initially to your field. You have to prescribe a initial field value otherwise it has to be read from a bc file

gregor

[maysmech]

Hi and thanks Gregor
I didn't find its format for vevtor DDtU with dimension [0 1 -2 0 0 0]. Do you know it?
Another question for Alberto:

DDtU =
fvc::ddt(U)
+ fvc::div(phi, U)
- fvc::div(phi)*U;

Are you mean DDt(rho*U)? because phi=rho*U and i think above relation is a material derivation of rho*U. Am i right?

[gregor]

try dimensionedScalar("ddtU", dimVelocity/dimTime/dimTime, 0.0)

edit: well obviously it has to be vector::zero instead of 0.0

[nimasam]

volVectorField DDtU
(
IOobject
(
"DDtU",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedVector("DDtU",dimensionSet(0,1,-2,0,0,0),vector::zero)
);
)

[maysmech]

Originally Posted by nimasam

volVectorField DDtU
(
IOobject
(
"DDtU",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedVector("DDtU",dimensionSet(0,1,-2,0,0,0),vector::zero)
);
)

Thanks Nima and Gregor
The problem is solved by:

    volVectorField DDtU
    (
        IOobject
        (
            "DDtU",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
    dimensionedVector("DDtU",dimensionSet(0,1,-2,0,0,0,0),vector::zero)
    );

But i am in doubt about DDtU value

DDtU = fvc::ddt(U) + fvc::div(phi, U) - fvc::div(phi)*U;

Is it DDt(rho.U)?

[nimasam]

no its not!!!!!! it is just DU/DT not D(rho U )/DT

[maysmech]

DDtU = fvc::ddt(U) + fvc::div(phi, U) - fvc::div(phi)*U

As it is stated in User guide phi=rho*U
So it has problem in dimension.

DDtU=>m/s2

ddt(U)=>m/s2

div(phi,U)=div((rho*U)U)=> kg/(m2s2)

div(phi)*U=> kg/(m2s2)

[maysmech]

Originally Posted by maysmech

DDtU = fvc::ddt(U) + fvc::div(phi, U) - fvc::div(phi)*U

As it is stated in User guide phi=rho*U
So it has problem in dimension.

DDtU=>m/s2

ddt(U)=>m/s2

div(phi,U)=div((rho*U)U)=> kg/(m2s2)

div(phi)*U=> kg/(m2s2)

i wrote above post because of:
http://www.openfoam.com/docs/user/fv...20-1120004.4.5

But phi which is written in time folders has this dimension: [0 3 -1 0 0 0 0]
And with this dimension it has dimension problem yet.

div(phi,U)=> m3/s2

[nimasam]

phi is not rho*U , it is U & sf()
sf() : surface vector
so
U (m/s) and sf (m^2) so phi is (m^3/s), ok?

[maysmech]

Ok, you mean it is not equal to what user guide wrote for phi. Maybe this is another phi.

But what is your idea about dimensional problem of DDtU?

[nimasam]

whats wrong with m/s^2 ?

[maysmech]

DDtU=>m/s2

ddt(U)=>m/s2

div(phi,U)=> m3/(s2)

div(phi)*U=> m3/(s2)

All of these four phrases should have same dimension, shouldn't they?