[gtarang]

Originally Posted by rahul62

Hi,
I am running the case (solidificationMeltingSource) in of4 but i am not getting alpha1 printed. Can anyone help me with this?

this fvoption uses sms1:alpha1, ie ':', colon in filename. If you are using openfoam in windows, then the file may not be written as windows does not allow ':' in filenames

[iconde]

Hi there,

I'm trying to get sms1:alpha1 variable for using it as a condition of a new variable in chtMultiRegionFoam but I'm having problems getting the variable because it doesn't recognize it:

./fluid/solveModuloTermicoFluid.H:18:28: error: ‘alpha1_’ was not declared in this scope
newVariable.ref() = alpha1_ * (dimensionedScalar("s", dimensionSet(0,0,1,0,0,0,0), scalar(1.0)));

/opt/openfoam6/wmake/rules/General/transform:25: recipe for target 'Make/linux64GccDPInt32Opt/chtMultiRegionFoamAzterlan.o' failed

Anyone knows how to call this variable?

Thanks!

[gtarang]

The variable alpha1_ will not be found directly as you are using. It is there in the memory but not in the .C or .H file in which you are calling.


First you have to search for the variable and then load it. Here you can go ahead in this direction:

volScalarField liquidFraction = this->mesh_.objectRegistry::lookupObject<volScalarField> ("sMS1:alpha1");

You may have to tweak the above code a bit to match the variable names present in the file.


You may also look at the documentation of chtmultiregionfoam on cpp.openfoam.org.


-gtarang

[iconde]

Thank you very much!

I've fixed the problem changing a little bit your function:

const volScalarField& liquidFraction = mesh.lookupObject<volScalarField>("sMS1:alpha1");

Thanks!!!!

[mikulo]

Originally Posted by gtarang

Hi,
I have been using solidificationMeltingSource as prescribed by you. Other than simple problems the solver fails and typically gives floating point exception error and runs for CFL no 0.1 or less for fine meshes.
I dug into the code and found that energy equation needs to be solved multiple times to actually correct the step function of liquid fraction as can be seen from the algorithm of Voller and Prakash (1987) http://dx.doi.org/10.1016/0017-9310(87)90317-6. I tried doing it by putting nEnergyCorrectors in PIMPLE dictionary and solving the energy equation n times. While I was debugging the code, I found this in solidificationMeltingSource.C line no 145.

if (curTimeIndex_ == mesh_.time().timeIndex())
    {
        return;
    }

Now according to my understanding, the above code ensures that the liquid fraction is updated only once and found it also. Can anyone suggest what can be the consequences of removing above bit of code.

Thanks
-
Tarang

Hello Tarang,

I have asked that same question too, seems like you are a mile ahead of me in PCM. I have seen your code too, where you remove the snippet above? May I ask, how was your result? Is there any change? It seems like mine is blowing up..

Thanks..

[gtarang]

I didn't remove that code. That code ensures that liquid fraction is updated only once in a timestep.


-Tarang

[mikulo]

Hello Tarang,

Yes, I understand you. However, if it is updated only once, then the liquid fraction is not corrected, right?Thus, I removed it and make some changes a little bit at the top level.

[Akshay_Ghorpade]

Hi Anna


In solidificationandMelting Source files (.C and .H) I am unable to understand the placement of this piece of code.



const volScalarField& liquidFraction = mesh.lookupObject<volScalarField>("sMS1:alpha1");

[kredosado]

Hi, I can run the case with bouyantFoam but when I try to use chtMultiRegionFoam the fvOptions "solidificationMeltingSource" does not work. Does anyone know why?

[mikulo]

Originally Posted by kredosado

Hi, I can run the case with bouyantFoam but when I try to use chtMultiRegionFoam the fvOptions "solidificationMeltingSource" does not work. Does anyone know why?

It will work, use the fvOptions for fluid region. Can I see your test case?

[kredosado]

[/QUOTE]

Originally Posted by mikulo

It will work, use the fvOptions for fluid region. Can I see your test case?

I've run it with fvOption. I want a sphere that may melt depending on the boundary condition. When I run it with these conditions for a temperature lower than the melting temperature, the sphere has some velocity. Plus the movingFront/alpha1 file I have set up doesn't appear in outside file 0. What could be the problem? For a 1 region case I have no problem running the melting source problem.

I cannot upload my case because it says security token is missing btw. And thanks in advance.

[calarcon]

Hi, I attached working melting gallium example running in openfoam11. In case someone needs to not work with a version from 15 years ago.

Launch like this

$ blockMesh
$ decomposePar
$ mpirun -np 8 foamRun -parallel > log &
$ reconstructPar
$ paraFoam

[Rakesh_Kumar]

Originally Posted by calarcon

Hi, I attached working melting gallium example running in openfoam11. In case someone needs to not work with a version from 15 years ago.

Launch like this

$ blockMesh
$ decomposePar
$ mpirun -np 8 foamRun -parallel > log &
$ reconstructPar
$ paraFoam

Hello Foamers
I want to capture the shrinkage void at air and solid(liquid) interface during solidification.
Does anybody know how to couple interFoam with this solidification solver????
If anybody has solver for this type of case, please share here
Or else, If anyone knows how to make this solver, please explain.


Currently, I'm struggling to setup my testcase for my thesis for this type of 3 phase.
Any sort of help regarding this problem is greatly appreciated.


Thanks in advance.

-Rakesh

[nando83]

Hi foamers,
I tried to run the attached example in openfoam-2312 but I got negative temperature with foam aborting.
I just added

	pRefCell 0;
	pRefValue 0.0;

to pimple setup in fvSolution.
Any idea of what's wrong here?
Thank you,

Nando

Originally Posted by calarcon

Hi, I attached working melting gallium example running in openfoam11. In case someone needs to not work with a version from 15 years ago.

Launch like this

$ blockMesh
$ decomposePar
$ mpirun -np 8 foamRun -parallel > log &
$ reconstructPar
$ paraFoam