OpenFoam 1.7.x, Gravity rotation for interFoam
 

Dear all
For OF 1.7.x, my "interFoam.C" looks like this with comments for my self (had to change it sligtly relative to the above discussion) Hope this is of help to someone! :)
NOTE: // a: //b: etc. marks the changes.

---------------------------------------------------------
#include "fvCFD.H"
#include "MULES.H"
#include "subCycle.H"
#include "interfaceProperties.H"
#include "twoPhaseMixture.H"
#include "turbulenceModel.H"
#include "interpolationTable.H"

// a:
#define pi 3.141592653589793238

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{

// b:
const dimensionedScalar gunits("gunits", dimensionSet(0,1,-2,0,0,0,0), 9.81);

#include "setRootCase.H"
#include "createTime.H"
#include "createMesh.H"
#include "readPISOControls.H"
#include "initContinuityErrs.H"
#include "createFields.H"


#include "readTimeControls.H"
#include "correctPhi.H"
#include "CourantNo.H"
#include "setInitialDeltaT.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Info<< "\nStarting time loop\n" << endl;

while (runTime.run())
{
#include "readPISOControls.H"
#include "readTimeControls.H"
#include "CourantNo.H"
#include "alphaCourantNo.H"
#include "setDeltaT.H"

runTime++;

Info<< "Time = " << runTime.timeName() << nl << endl;

// ------------------
// kemur fra creatFields.H, virdist breyta litlu ad hafa thetta a:
// dimensionedVector g0(g);
// ------------------

// c:
// the file ./constants/g seems to be overwritten or ignored.
// Have tested by setting gravity to -0.05 m/s2 as well as -99.8 m/s2 in
// ./constants/g => same result is produced regardless! I.e. the line
// below seems to dominate over anything that is written in ./constants/g.
g=gunits*Foam::sin(runTime.value()*pi/2.0)*vector(1,0,0)-gunits*Foam::cos(runTime.value()*pi/2.0)*vector(0,0,1);

// ------------------
// Comes from creatFields.H, virdist breyta litlu ad hafa thetta a:
// dimensionedVector g0(g);
// ------------------

// --------- from createFields.H
// d:
// Comes from the file createFields.H. You dont have to delete the lines
// in createFields.H. The field gh is just initilaized there.
Info<< "Calculating field g.h\n" << endl;
volScalarField gh("gh", g & mesh.C());
surfaceScalarField ghf("ghf", g & mesh.Cf());
// -------------------------------------


twoPhaseProperties.correct();

#include "alphaEqnSubCycle.H"

#include "UEqn.H"

// --- PISO loop
for (int corr=0; corr<nCorr; corr++)
{
#include "pEqn.H"
}

turbulence->correct();

runTime.write();

Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
<< " ClockTime = " << runTime.elapsedClockTime() << " s"
<< nl << endl;
}

Info<< "End\n" << endl;

return 0;
}

This thread is a bit old but hopefully someone could help....

i have the same problem, wanna change g and make it as a function of time. I have OF 2.1 and in interFoam solver file i cant find the file : readGravitationalAcceleration.C ... I tried to change the interFoam.C file like diescribed above but it didnt work (i ran interfoam as normal on a test case and it just takes the constant value of g in "constant" file)... i tried to write the codes in creatFields.H but it didnt work either (again interFoam runs normal with no changes as if i didnt change anything in the code).

I would really appreciate some help or advice

Thanks

interFoam 2.1.x Rotation
 

Hi Callahance

I just compiled gravity rotation into interFoam 2.1.x. The files needed to be changed/modified are the interFoam.C and the UEqn.H

here are my modifications (search for VVPF in interFoam.C and UEqn.H) to see the changes.

Note that this compile without any problems, but I haven't had time to test the binaries. Hope this is enough to get you started:)

cheers
JonW

JonW... all what i could say is : THANKS... ill try it out and give a feedback... thanks very much again

Hey Claus,

Hello. This is a very old post. Its feels quite strange to ask a question now. Please bear with me. I want to know how the code worked since you never defined the variable 'g'. I'm trying to do something similar for a plunging airfoil. I get an error " In function ‘int main(int, char**)’: , ‘g’ was not declared in this scope "

If you no longer remember thats OK.

Thanks,
Pru.

you have to define g in createFields.H with the #include "readGravitationalAccelation.H" - thingi (see the createFields.H in the interFoam solver).

If you are going to use gravity in a single phase fluid, check out
http://www.cfd-online.com/Forums/ope...interfoam.html

J.

Heaving reference frame
 

Hey john thanks for the reply!

I'm simulating a flapping airfoil and I want to use a heaving reference frame instead of using a deforming mesh. This means that the fluid should accelerate up and down in a sinusoidal motion. So I changed the Ueqn as follows

I defined max_ acceleration and frequency in createFields.H as follows

When I do wmake I get the following error.
However Claus managed to run his code.

I want to know where I went wrong in the process. I will check out the link you mentioned.

i made it whyman........ simply enter following code in your creatFields.H


// Read the data file and initialise the interpolation table
interpolationTable<vector> timeSeriesAcceleration
(
runTime.path()/runTime.caseConstant()/"acceleration.dat"
);
g.value() = timeSeriesAcceleration(runTime.value());

compile it

and then make an acceleration.dat file in your constants case directory in following format

4
(
(0 (1000 0 0))
(3 (1000 0 0))
(4 (1000 0 0))
(5 (12000 0 0))
)

run the case and enjoy

I tried to specify acceleration from file acceleration.dat file. but there is a problem. solver gets only first value of acceleration and after that it dont read acceleration.dat file. i added following code in interfoam creatFields.h

// Read the data file and initialise the interpolation table
interpolationTable<vector> timeSeriesAcceleration
(
runTime.path()/runTime.caseSystem()/"acceleration.dat"
);
g.value() = timeSeriesAcceleration(runTime.value());

please try and help me too......

createFields.H is just read at the beginning of the simulation. You should update g.value() at each time step

ya i know problem is creatfields.h is read once but......
 

yes boss i know creatFields.H is read just once. and i have to update g.value at each time step.... but the problem is how to do it..... i have tried by adding while loop in creatFields for g.value() but it doesnt work. as you said creatFields is read only once. if i take out g.value form creatFields.H and place it in interFoam g.value does not replace g vector specified in constants directory of the case. please suggest if you have an idea.....

While loops in createFields.H doesn't make sense, since the timeStep isn't updated. Update g.value() in runTime while loop (interFoam.C).

For example:

sir i tried this but it doesnt solve for acceleration from acceleration.dat instead it solves from g file. i have already tried this.....

i have tried it by keeping g.value() = timeSeriesAcceleration(runTime.value()); at the same place as you kept... but doing this solver stops taking value from acceleration.dat it takes g value from g file. as it solves g in creatFields for gh and p_gh both gets g value.....

any other suggestion sir???

then you should update gh and ghf, too.

thank you sir it works

Hi，clause. Your answer to changable acceleration seems correct, but how can I handle the g file in const folder. Thanks in advance.

no match for operator error in implementing variable gravity
 

Based on the direction given in this thread,

I tried using the line
g=gunits*vector(0,Foam::sin(runTime.value()*pi*2.0 *freq),1) for sinusoidal lateral acceleration


I get an error

interFoam2.C:114:3: error: no match for âoperator=â (operand types are âconst Foam::meshObjects::gravityâ and âFoam::dimensioned<Foam::Vector<double> >â)
g=gunits*vector(0,Foam::sin(runTime.value()*pi*2.0 *freq),1);

I also tried the line given in the thread as such to test. That too gave a similar error. Am I missing some step? I do hope I get a response considering that this is an very old thread.

I am using v1812

I dont think you can put the "Foam::"-thingi into vector()
Rather try this,...
g=gunits*Foam::sin(runTime.value()*pi*2.0*freq)*ve ctor(0,1,0) + gunits*vector(0,0,1);


If this is indeed gravity, make sure that abs(g) = 9.81. Like this vector is now, then its not the case.
Hope this helps.