[kera]

Originally Posted by akidess

Sen and Davis do not present experimental results if I remember correctly. The results in that paper are based on a semi-analytic model. Based on what you put in you will obtain other results. What were the values you expected, for which dimensionless numbers?

Yes, you are once again right , and sorry for not being clear with the information.

Like I said, I tried to recalculate the properties of the fluid from the given dimensionless numbers for the case Mg = 0.2, Ca = 0.008, Re = 1 and Pr = 0.2 (Also assuming both fluids have same properties).

I have also attached my case file with those values, I am not sure about the values though but I hope it is still plausible to do so.

Thanks once again in advance!

Regards,
Ricky

[akidess]

Originally Posted by kera

(Also assuming both fluids have same properties).

Pretty sure that assumption is not valid. Did you read the Sen and Davis paper?

[kera]

That is the problem, currently I don't have accces to their research work, so I tried to gather as much information as possible from the available resources on the internet and obviously most of the data is still missing. I did place a request to get access to their research work but I have no idea how long it is gonna take, that pretty much gave me a reason to post the query here.

[akidess]

Originally Posted by kera

That is the problem, currently I don't have accces to their research work, so I tried to gather as much information as possible from the available resources on the internet and obviously most of the data is still missing.

OK, that explains a lot... Still, Zaki's thesis clearly states there is a gas on top of the liquid - odd choice you assume both fluids to have the same properties (Sen and Davis go a step further and assume a fluid of negligible viscosity and thermal conductivity).

[vak96]

Hi all,

I am new to OpenFOAM. I am working on solidification of ingot during vacuum arc remelting. I tried using all the above solvers but none of them seems to work as I am getting an error while compiling. I am using OpenFOAM version 2.3.0. Can someone please help me?

Thanks in advance,
Akshay

[kera]

Originally Posted by vak96

Hi all,

I am new to OpenFOAM. I am working on solidification of ingot during vacuum arc remelting. I tried using all the above solvers but none of them seems to work as I am getting an error while compiling. I am using OpenFOAM version 2.3.0. Can someone please help me?

Thanks in advance,
Akshay

Hi Akshay,

I am not sure what kind of compilation errors you are talking about, if I have to guess those errors are probably due to version mismatch.

Have you tried using the "solidificationMeltingSource" fvOption which comes with OpenFOAM (not sure about 2.3.0 but it's definitely present from 2.3.1 onwards )? I haven't used it myself though, but you can refer to #218 for a sample case (pay attention to the version).

Also, if I remember it correctly someone has uploaded his/her solver for OpenFOAM-2.3.0.

Happy FOAMing!

Regards,
Ricky

[vak96]

Hi Ricky,

Thanks for your help. I will try and get back to you if I have any problem.

Regards,
Akshay

[vak96]

Hi guys,

I have tried finding out how to use "solidificationMeltingSource" fvOption in #218 but was not successful. Can anyone please provide me with some tutorial case with geometry?

Thanks in advance,
Akshay

[kera]

Originally Posted by vak96

I have tried finding out how to use "solidificationMeltingSource" fvOption in #218 but was not successful.

Hallo Akshay,

Sorry for the late reply, I was stuck with documentation .

As far as your problem is concerned, it would be helpful if you can elaborate what you tried to do and where exactly you are encountering compilation errors. After my last post I was curious enough to try that "fvOptions" myself and it worked out pretty much good for me.

The tutorial case provided in post #218 is for the OpenFoam-Version 3.0 and you would definitely end up with errors if you try to run that case with your OpenFOAM-Version 2.3.

The usage of "solidificationMeltingSource" is slightly different in version 2.3 when compared to version 3.0.

Hope this helps!

Regards,
Ricky

[vak96]

Hi Ricky,

I was able to run it OpenFOAM version 4.1. Can you please elaborate the usage of "solidificationMeltingSource" with respect interfoam solver which uses VOF method. Whether such thing is possible or not?

Thanks for the previous reply.

With regards,
Akshay

[kera]

Hallo Akshay,

To be honest, I have really no clue about it.

If I am not overthinking it there is no direct way to use solidificationMeltingSource with interFoam for the following reasons:

• solidificationMeltingSource term for the time being doesn't handle two phases (atleast not in OpenFoam-2.3.1) So you have to program it.
• InterFoam being an isothermal solver you need to add energy equation (which is quite easy to add).

After adding the energy equation to interFoam I would definitly try the solidificationMeltingSource term by setting alpha=1 for the whole domain (solving it as a single phase) I don't think it would work but still just to get an idea.

If you are very keen about modifying the solidificationMeltingSource term. I would also look into the "OpenFOAM-2.3.x/src/transportModels/incompressible/" so as to modify/append the solidificaitonMeltingSource by incorporating VOF calculations -- If it is plausible.

(or)

You can go ahead and implement the melting algorithm by Fabian directly in interFoam.

Any help from others is really appreciated.

Regards,
Ricky

[vak96]

Hi all,

I have shared a folder which has a tutorial along with solver and a test case.https://drive.google.com/file/d/0Bzj...ew?usp=sharing
I have tried to do what this document says to make our own solver based on interphasechangefoam with temperature term included in OpenFoam version 4.1. When I compiled the solver there were no errors but when I do solver -help or run it, it shows the following error. Can anyone help, please?

Thanks in advance,
Akshay

[kera]

Originally Posted by vak96

Hi all,

I have shared a folder which has a tutorial along with solver and a test case.https://drive.google.com/file/d/0Bzj...ew?usp=sharing
I have tried to do what this document says to make our own solver based on interphasechangefoam with temperature term included in OpenFoam version 4.1. When I compiled the solver there were no errors but when I do solver -help or run it, it shows the following error. Can anyone help, please?

Thanks in advance,
Akshay

Hallo Akshay,

Double free or corruption means either you are deleting the same entity twice or deleting unallocated memory.

I see that you are also compiling the libraries associated to interPhaseChangeFoam once again in your FOAM_USER_APPBIN and seems to me that is actually causing the error.

Just replacing your "Make/file" with the following should solve your problem.

myInterPhaseChangeFoam.C 

Exe = $(FOAM_USER_APPBIN)/myInterPhaseChangeFoam

Regards,
Ricky

[zzj]

[QUOTE=fabian_roesler;329995][FONT=&quot]Hi

hello,fabian,your solver really works,but I have some questions about your solver.You define a variable named rhok,then add an annotation:Kinematic density for buoyancy force.
There is little information about the variable. I really can not figure out what kinematic density means,could you give me some suggestions?

[kera]

[QUOTE=zzj;637726]

Originally Posted by fabian_roesler

[FONT=&quot]Hi

hello,fabian,your solver really works,but I have some questions about your solver.You define a variable named rhok,then add an annotation:Kinematic density for buoyancy force.
There is little information about the variable. I really can not figure out what kinematic density means,could you give me some suggestions?

I hope this helps!

https://openfoamwiki.net/index.php/B...sinesqPisoFoam

Ricky

[zzj]

[QUOTE=kera;637754][QUOTE=zzj;637726]

hi, Ricky

thanks a lot,it really helps.

The essay gives a detailed explaination so that I can understand.

zzj

[cfd@kgp]

Originally Posted by fabian_roesler

Hi

Actually you do not have to compile anything, as the whole solver for solidification and melting is there as a new fvOption module since version 3.

Check this out:
http://cpp.openfoam.org/v4/a02447.html#details

Cheers

Fabian

Hi Fabian and all phase-change foamers,

The solidification and melting sources (in OF 3.x and 4.x ) gives accurate transient results. I have checked both the transient meltfront evolution and the time evolution of Nusselt numbers for melting.

However, the definition of fluid fraction do not seems to convince me, especially values of fluid fraction cannot be correlated with the temperature,

forAll(cells_, i)
{
label cellI = cells_[i];

scalar Tc = T[cellI];
scalar Cpc = Cp[cellI];
scalar alpha1New = alpha1_[cellI] + relax_*Cpc*(Tc - Tmelt_)/L_;

alpha1_[cellI] = max(0, min(alpha1New, 1));
deltaT_[i] = Tc - Tmelt_;
}

can any body explain me the rationale of this fluid fraction defination---> Cpc*(Tc - Tmelt_)/L_;

Any Research paper with this definition?

Fabian your advice is very much needed. Please help.

Thanks in advance!

[gtarang]

 Cpc*(Tc - Tmelt_)/L_

It basically gives the amount of energy contained in the fluid cell above melting point and then we divide it by L to get the fraction. If Tc < Tmelt, we get negative value and then we constrain the alpha to 0 similar things happen when alpha becomes greater than 1, we constrain it to 1.
However, based upon the Voller et al. of papers of phase change, I think Tc should be constraint to Tsolidus or Tliquidus (or Tmelt) when 0<alpha<1 and Tc is out of range of Tsolidus and Tliquidus.
After simulations with different materials I have seen that for alpha still within (0,1), T > Tmelt. I am right now trying to see what can be done about it.

[Typhain]

Hello everyone. I'm interesting about solving melting/solidification problems on openFoam and that's why I'm trying to adapt conMeltFam parallel solver fo 5.0 version.

But there is a probleme when compiling it. In the header Teqn.H, there is a probleme when using gMax and gSum:

residual = gMax(mag(alpha3New.internalField()-alpha3.internalField()));
meanResidual = gSum(mag(alpha3New.internalField()-alpha3.internalField())*mesh.V())/gSum(mesh.V().field());

And the error message is the folowing

TEqn.H:37:78: error: no matching function for call to ‘gMax(Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> >)’

Then I thought it was due to dimension of alpha3 and alpha3New so I built a forAll loop like that

	forAll(alpha3,i)
	{
	forAll(alpha3New,i)
	{
        residual = gMax(mag(alpha3New[i]-alpha3[i]));
        meanResidual = gSum(mag(alpha3New[i]-alpha3[i])*mesh.V())/gSum(mesh.V().field());
	}}

But then it say that

error: no matching function for call to ‘gMax(Foam::doubleScalar)’

So I am a little bit confuse about gMax function, what should be the dimension of alpha3 to use it ?

thanks

[cfd@kgp]

Hi Typhain!

If I am not wrong convMeltFoam was developed for version 2.0 or 2.1.0 I have to see the exact version.

So there have been various changes in foam files. were you successful to compile the solver in OF4.0 or OF3.0 or OF2.4 or OF2.3 or OF2.1? these are some of the major releases (many changes in each step).

The conventional way is to climb one step at a time.

upload your solver and mention the compatible solver version. So we will try to upgrade it step by step till current version.

Thanks!