[sahmed]

Hello Foamers
I need your suggestion regarding a very interesting and useful topic. Suppose I got a fully-developed velocity profile from a pipe flow solution (U Vs. Z) and I want to implement it to another problem as an initial velocity field. This might save some of the computational time since the solver is already dealing with a good solution.
Did anyone use this type of condition in any of your simulations?? ANY type of suggestion is highly appreciated.

[sahmed]

Anybody please give me some hints from your experience how to add my own initial conditions to a problem, say an initial temperature profile or an initial velocity profile

[alexeym]

User Guide, chapter 2.1.5.3. In fact whole section 2.1.5 could be useful - http://cfd.direct/openfoam/user-guid...#x5-170002.1.5.

[sahmed]

Thanks Alexey. I was thinking of using somehow the setFields utility to specify a user-defined initial velocity of temperature profile. This might be the easiest option if I can do that.
Not necessarily that I have to merge the older one with the new one as you mentioned. Suppose that I have any profile and I want to use it as my initial condition instead of a fixed value.

PLEASE help me if you have any idea.

[alexeym]

Well, you can use setFields, you can use codeStream as internalField (if you know OpenFOAM's C++), you can use so called funkySetFields (according to forum it can be used for the case you have described, yet I have never used it myself). Below is an example of codeStream as internalField for velocity:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}

dimensions      [0 1 -1 0 0 0 0];

internalField   #codeStream
{
    codeInclude
    #{
        #include "fvCFD.H"
        #include "vectorField.H"
    #};

    codeOptions
    #{
        -I$(LIB_SRC)/finiteVolume/lnInclude \
        -I$(LIB_SRC)/meshTools/lnInclude
    #};

    code
    #{
        const IOdictionary& d = static_cast<const IOdictionary&>(dict);
        const fvMesh& mesh = refCast<const fvMesh>(d.db());
        vectorField U(mesh.nCells());
        const vector C = vector(0.05, 0.05, 0.005);
        forAll(U, i)
        {
            const vector& Ci = mesh.C()[i];
            const vector R = Ci - C;
            U[i] = R ^ Ci;
        }
        U.writeEntry("", os);
    #};
};
...
[your boundary conditions]

Since your description of the problem is rather vague, there are plenty of possibilities. "Any profile" proposes random solution.

[ancolli]

Originally Posted by alexeym

Well, you can use setFields, you can use codeStream as internalField (if you know OpenFOAM's C++), you can use so called funkySetFields (according to forum it can be used for the case you have described, yet I have never used it myself). Below is an example of codeStream as internalField for velocity:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}

dimensions      [0 1 -1 0 0 0 0];

internalField   #codeStream
{
    codeInclude
    #{
        #include "fvCFD.H"
        #include "vectorField.H"
    #};

    codeOptions
    #{
        -I$(LIB_SRC)/finiteVolume/lnInclude \
        -I$(LIB_SRC)/meshTools/lnInclude
    #};

    code
    #{
        const IOdictionary& d = static_cast<const IOdictionary&>(dict);
        const fvMesh& mesh = refCast<const fvMesh>(d.db());
        vectorField U(mesh.nCells());
        const vector C = vector(0.05, 0.05, 0.005);
        forAll(U, i)
        {
            const vector& Ci = mesh.C()[i];
            const vector R = Ci - C;
            U[i] = R ^ Ci;
        }
        U.writeEntry("", os);
    #};
};
...
[your boundary conditions]

Since your description of the problem is rather vague, there are plenty of possibilities. "Any profile" proposes random solution.

I am having the following Error in OpenFOAM-dev

error: ‘Foam::vectorField {aka class Foam::Field<Foam::Vector<double> >}’ has no member named ‘writeEntry’
/opt/openfoam-dev/wmake/rules/General/transform:25: recipe for target 'Make/linux64GccDPInt32Opt/codeStreamTemplate.o' failed
make: *** [Make/linux64GccDPInt32Opt/codeStreamTemplate.o] Error 1

however, in OpenFOAM-6 is working well.

[Carlo_P]

A very simplem method can be copy and paste the value in the oldSim/U to the nuew 0/U.


If the mesh is different, you can easily apply a mesh conversion