[usv001]

Hi Bruno,

Thanks for replying once again. I actually have two versions of OF installed (2.1.1 & 2.4.1). I was able to run the incompressible/simpleFoam/pipeCyclic test case in both versions successfully. However, since my ParaView is linked to v2.1.1 only, I am able to view the results only when I run the solver using v2.1.1 but I can see that the swirl has been implemented in both version by looking at the result files.

At time=0, ParaView does not show the swirl boundary condition. So, you were right the first time: the BC is not reflected in ParaView at t=0 but passed to the solver during the first time step or during decomposePar.

[My Linux distribution information
Distributor ID: Ubuntu
Description: Ubuntu 12.04.5 LTS
Release: 12.04
Codename: precise

I tried to run my own case and I was able to run it without any problems in v2.4.1 (I'm using rhoCentralFoam). I checked the results by checking the results files and the code has been implemented. Just some observations:

(1)
Both...

operator == (200000);

and...

operator==(200000);

worked.

(2)
I removed the following statements since they were absent in the pipeCylic tutorial and it worked fine:

        codeInclude
        #{
        #include "fvCFD.H"
        #};

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

(3)
When I added the #include statements, I got the following error after the first iteration:

#0  Foam::error::printStack(Foam::Ostream&) in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigSegv::sigHandler(int) in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::fixedValueFvPatchField<double>::gradientInternalCoeffs() const in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::codedFixedValueFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#6  ? in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  ? in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
Segmentation fault (core dumped)

I am not too sure why this happens but would love to understand if anyone knows.

Many thanks to everyone and especially, Bruno.

[wyldckat]

Quick answers:

Originally Posted by usv001

(1)
Both...

operator == (200000);

and...

operator==(200000);

worked.

Mmm... strange... I thought C++ demanded the operator methods to be written without spaces in their name, such as "operator==". Very strange.

Originally Posted by usv001

(2)
I removed the following statements since they were absent in the pipeCylic tutorial and it worked fine:

        codeInclude
        #{
        #include "fvCFD.H"
        #};

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

(3)
When I added the #include statements, I got the following error after the first iteration:

#0  Foam::error::printStack(Foam::Ostream&) in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigSegv::sigHandler(int) in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::fixedValueFvPatchField<double>::gradientInternalCoeffs() const in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::codedFixedValueFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#6  ? in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  ? in "/home/cae-usv/OpenFOAM/OpenFOAM-2.4.0/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
Segmentation fault (core dumped)

I am not too sure why this happens but would love to understand if anyone knows.

"sigSegv" - segmentation fault, probably due to a bad memory access. It's even stranger that it happened within "gradientInternalCoeffs".

Did you change anything in the original source code files within OpenFOAM's source code?

[usv001]

Hi Bruno,

No, I have not changed any original source code files.

[SmokedJuggler]

Hello All,

I am interested in applying an unsteady and non uniform boundary condition for inflow.

I want to define a function for the velocity profile such as:

U(x)=U_0*(exp(y)*sin(2*pi*freq*time))

where y is the vertical position of inflow patch in a channel. I want to avoid using groovy boundary condition.

I would appreciate if any one could also help me with this.

Regards

[usv001]

Hi Sam,

I managed to get the code below working following what was suggested earlier on this thread. It is a parabolic velocity profile.

INLET
    {
        type            codedFixedValue;
	value 		uniform (0 0 0);
	redirectType	test; // user-defined name

	code
	#{
	const fvPatch& boundaryPatch = this->patch(); 
        const vectorField& Cf = boundaryPatch.Cf(); 

        vectorField& v = *this;
        scalar Uc = 1; // centerline velocity, U_max
	scalar R = 0.019; // inlet radius

	forAll(Cf,faceI)
	{
	    scalar x = Cf[faceI].x(), y = Cf[faceI].y(), rSq = x*x + y*y;
            v[faceI] = vector(0, 0, Uc*(1 - rSq/R/R));
	}
        #};
}

You can try modifying it. I think you can start with the following. I have not tried running though.

INLET
    {
        type            codedFixedValue;
	value 		uniform (0 0 0);
	redirectType	test; // user-defined name

	code
	#{
	const fvPatch& boundaryPatch = this->patch(); 
        const vectorField& Cf = boundaryPatch.Cf();
        const scalar &t = this->db().time().value();

        vectorField& v = *this;
        scalar U0 = 1; // centerline velocity
	scalar f = 1; // frequency

	forAll(Cf,faceI)
	{
	    scalar y = Cf[faceI].y();
            scalar u = U0*Foam::exp(y)*Foam::sin(Foam::constant::mathematical::twoPi*f*t);
            v[faceI] = vector(u, 0, 0);
	}
        #};
}

All the best!

[smodh]

Hello Foamers,

I want to implement a boundary condition at electrode.

N_P= K * Efield * N_P


In this equation N_P and Efield " need to be taken from electrode at previous time step and K is dimensionedScalar fix value 1.

is there anyone know how to implemrnt this BC? should I have to used codedfixed BC or some other BC? I am using openfoam 4.0.

Thanks in advance.....

[smodh]

Hello Foamers,

I want to implement a boundary condition at electrode.

N_P= K * Efield * N_P


In this equation N_P and Efield " need to be taken from electrode at previous time step and K is dimensionedScalar fix value 1.

is there anyone know how to implemrnt this BC? should I have to used codedfixed BC or some other BC? I am using openfoam 4.0.

Thanks in advance.....

[kuria]

Thank you for the information on implementing time in the boundary condition!


I was wondering if someone has looked into how to import time step used by the solver while calculating the boundary condition using CodedFixedValue or Codedixed?


Thanks in advance

[usv001]

Originally Posted by kuria

I was wondering if someone has looked into how to import time step used by the solver while calculating the boundary condition using CodedFixedValue or Codedixed?

Hi Kurian,

Simply use the following to obtain the time step.

const scalar &t = this->db().time().deltaTValue();

Best,
USV

[kuria]

Originally Posted by usv001

Hi Kurian,

Simply use the following to obtain the time step.

const scalar &t = this->db().time().deltaTValue();

Best,
USV

Hey


Awesome, that was perfect!
Thank you

[arashfluid]

Dear friends,
I am solving the flow around the sphere (as a particle) inside a channel. I want to calculate the integral of the drag force over the sphere at each time step to calculate the velocity of the sphere V2 (F=m.(V2-V1)/dt) and then applied the obtained velocity (V2) at each time step to the inlet boundary as a portion of velocity boundary condition (U-V2). How can I do this?