Solidification in OpenFoam
 

Dear all,

I'm going to use OpenFoam for simulating a continuous casting problem. I'm completely new to OpenFoam, and it seems to me that there is not any solidification model in OpenFoam. Should I create solidification model myself?

As my case is continuous casting, I should consider a pull velocity for solid phase, too. Is it possible without great difficulties in OpenFoam?

I will be thankful for you reply.

Updates
 

Are you still interested in solidification in OpenFOAM?

Hello

I'm newbie with OpenFOAM, but I'm interested to model solidification of steel. If i have well understood, there is no built-in solver? Do you know where I can find one?

Regards

solidification problem
 

Hi

In the thread http://www.cfd-online.com/Forums/ope...g-problem.html you can find several solvers for melting and solidification using the enthalpy method and the enthalpy porosity method.

Regards

Fabian

Thanks a lot

Explanation for terms in TEqn.H?
 

Hello all!
I am trying to use meltFOAM for my project on solidification of lavas. I am trying to understand the terms appearing in TEqn.H. I identified the dT/dt, advection and diffusion terms, and then see terms that involve latent heat, and what I figure is some sort of a melt fraction term, but I don't understand the details -- what is the exponent, where did all the "4" factors come from, etc.?
Here's the code:

fvScalarMatrix TEqn
(
fvm::ddt(cp, T)
+ fvm::div(phi*fvc::interpolate(cp), T)
+ hs*4.0*exp(-pow(4.0*(T-Tmelt)/(Tl-Ts),2))/Foam::sqrt(pi)/(Tl-Ts)*fvm::ddt(T)
+ hs*4.0*exp(-pow(4.0*(T-Tmelt)/(Tl-Ts),2))/Foam::sqrt(pi)/(Tl-Ts)*(U & fvc::grad(T))
- fvm::laplacian(lambda/rho, T)
);

Thanks!!!

Have a look into my paper on the solver:

F. Rösler, D. Brüggemann (2011): Shell-and-tube type latent heat thermal energy storage: numerical analysis and comparison with experiments. Heat and Mass Transfer, Vol. 47 Issue 8 , 1027-1033, DOI: 10.1007/s00231-011-0866-9
http://www.springerlink.com/content/b1tp01k2u7q8j432/

Keep in mind that the solver does not account for non-linearity like the linear source method by Voller. The erfMeltSolver just reduces the non-linearity effects in the energy conservation equation. For simple problems, the results converge with a very small error for the energy conservation. With increasing convective transport, the error increases and some iteration to account for the non-linearity have to be performed.
In my previous work, I use a linear liquid fraction function and the linear source method proposed by Voller.

Regards

Fabian

Excellent paper Fabian! Thanks for pointing it. Just what I needed.

Stefan problem
 

Sir
i am also trying to analysize the phase change problem.I want to know is it possible to do it on Fluent and if yes which solver /model i should go for.
thanks

Hi dinesh

Yes, Fluent offers an Enthalpy-Porosity-Method for simulation of solid/liquid phase change. Unfortunately I never used Fluent for such simulations so go on and find out yourself. Good luck.

Regards

Fabian

Hello danish.

As Fabian said, FLUENT can solve Solidification/Melting problems. I myself tested and validated the solver for my thesis. There are excellent tutorial and theory materials from Ansys Fluent. Using Google, you may find them with no problem.

Have fun!

I found from literature but there is contradiction.
Ref "H. Shmueli et al. / International Journal of Heat and Mass Transfer 53 (2010) 4082–4091" this paper says "page number 4086 says: As for the pressure discretization, only PRESTO!and Body-Force-Weighted schemes are available for the VOF and mixture multiphase models." Does this means that multiphase has to be used for my case. Enabling this i find that courant number can be inserted which the paper says to be kept around 0.5. what about the phase 1 and phase 2. see this post by me which flotus replied on 11july
Ref "http://www.cfd-online.com/Forums/system-analysis/120322-stefan-problem.html#post439934"
eagerly waiting for the reply

So you have two zones, one is a closed container with PCM solidification and the other with a fluid flow around container, Right? If so, you don't need multiphase model at all. Using Fluent, during the solidification there is only one phase (fluid). To model solid zone (which is not really a solid phase in this model), Fluent adds a huge artificial viscosity to the solid zone to prevent flow on it. In this way, there is no need to define two phase flow.

I think this open access paper can help you:
A Numerical Study on Time-Dependent Melting and Deformation Processes of Phase Change Material (PCM) Induced by Localized Thermal Input

I went through this paper it refers on page no 529 TO REPRESENT THE FREE SURFACE OF THE MELTING REGION ADJACENT TO THE GAS PHASE, VOF METHOD IS USED. Now in fluent this VOF is under the menu of multiphase model. so plz clarify me? how can i find the melted region profile?

You didn't answer my question about whether the solidification zone is a fully filled container or not? If there is no gas in contact, using VOF is not necessary at all.
When you plot the contour of liquid fraction (F) the melt-solid (or melt-gas) interface can obviously be seen and extract. Refer to Kim's paper, Fig. 9 to 11.

I am handling without air case.
Plz see the plot i got
https://www.dropbox.com/s/gg3mqyum1u3mx5z/frac4000s.png
How can i extract the data regarding the anount or percent of solid melted/or mushy zone volume.
thanks

You need to calculate volume integral of liquid fraction. Fluent can do this by some simple Clicks. Do as below:
-From Menu Bar, go to Report and choose Volume Integrals... to open Volume Integral Window.
-In Volume Integrals Window:
--Choose Fluid (or whatever the solidification zone's name is) from right menu (Cell Zones),
--Choose Volume Integral from left menu (Report Type),
--Under Field Variable, select Solidification/Melting... and then Liquid Fraction,
--Click Compute button... and it's done!
Good Luck

thankyou very much for the support you provided.
Can you plz tell me about the discretization method. I used SIMPLE method with PRESTO scheme (without gravity being aplied) i got some result. Now i am using PISO with Body Force weighted with gravity added slowly from 1m/s2 to 9.81 m/s2 (as recommended by some user). I run the simulation for some time and then i get divergence either in epsilon or( x y z componenet of velocity) can you suggest some way to overcome this.

What are Ra and Pr numbers related to your simulation?

I've done an unsteady simulation of melting Gallium in a 2D cavity with Ra=2.2x10^5. I used SIMPLE for pressure-velocity coupling, PRESTO! for pressure discretization and SST k-w for turbulence modeling. You can obtain a good convergence with a small enough time step and fine enough grid.

If the convergence problem is still bothering, bring up more info about your simulation.

With SIMPLE and PRESTO i also got the convergence. But with PISO and Body Force weighted i am not getting the convergence, I am refering" H Shmueli et al /IJHMT 53(2010) 4082-4091 where he is comparing the different schemes(page no 4085).
Regarding Pr and Ra i have not calculated. My hot water flow velocity is 0.1m/s at 350 K which is used to melt parafin wax which initially is at 293K and melting temperature is 313-316K. Hot fluid flows inside while the outer cylinder(0.6m dia 1m length) is enclosing the wax.

If so, why are you using PISO and Body Force Weighted?

I think the problem is not using SIMPLE or PISO / PRESTO! or B.F.W.
Reduce all under relaxation factors to 0.5. Finer meshes or smaller time steps also may provide a converged solution.

Have you tried SST k-w instead of k-e?

I am trying to validate my model with the "shumeli model" with gives the comparision of these two models.
Also the reason of using k ep model is that it has enhanced wall function,My model contains circular fins. so i went with that.
Reducing the URF helps in convergence but i thk we must not alter these values as they effect the results.
Can you suggest about some rule for governing the grid size?

k-ep is a very inaccurate model for near wall regions. The standard turbulence model for general purpose simulations is SST k-w. You can find the reasons in any up to date turbulence text and in CFX documentations, too.

Changing URFs affects the way the solution converges, but after achieving a converged solution (small enough residuals, with monotonic residual curves) it doesn't matter how you've done it. Generally speaking, reducing URFs provide a better convergence, but more run time is required.

Start with a coarse mesh and make it finer and finer till the results are not changed (Grid Independency Test)

Dear Sir
Can you suggest: while using Boussinesq parameter under operating condition menu, what should be the operating temperature and operating density. (Should it be The melting temperature and the solid state density of phase change material or something else)
Also plz suggest, since we have in governing equation additional source terms in the momentum and energy equations, so how do we calculate these values. Regarding input in the fluent there is option under cell zone conditions/ checking the source terms enable us to enter these values of mass, momentum, energy source term. But how do I calculate it from governing PDE.

An estimation of operating temperature can be the average of maximum and minimum temperatures in system. This is also applicable for density.

When you enable Solidification model in Fluent, related source terms are implemented into equations automatically. You need not to import anything.