# Solid/liquid phase change

 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 13, 2009, 09:35 Solid/liquid phase change #1 Senior Member     Fabian Roesler Join Date: Mar 2009 Location: Bad Friedrichshall, Germany Posts: 161 Rep Power: 8 Dear Foamers For a project I am trying to get a solid/liquid phase change simulation running in OF 1.5-dev. A paraffin with non isothermal phase change is molten in a 2D rectangular test case scenario. I started from interFoam solver by changing especially the gamma equation to my needs: Gamma equation: dimensionedScalar pi = mathematicalConstant:i; dimensionedScalar alpha = (Tl-Ts)/(scalar(2)*tan(scalar(0.49)*pi)); gamma = atan(scalar(1)/alpha*(T-(Tl+Ts)/scalar(2)))/pi+scalar(0.5); Changig gamma from 0 (solid) to 1 (liquid) depending on the temperatures Tl (upper phase change temperature) Ts (lower phase change temperature) Momentum equation: fvVectorMatrix UEqn ( fvm::ddt(rho, U) + fvm::div(rhoPhi, U) - fvm::laplacian(muf, U) - (fvc::grad(U) & fvc::grad(muf)) ); UEqn.relax(); if (momentumPredictor) { solve ( UEqn == fvc::reconstruct ( ( - ghf*fvc::snGrad(rho) - fvc::snGrad(pd) ) * mesh.magSf() ) ); } No changes at all, however no surface tension left Energy equation: volScalarField rhoCp("rhoCp", rho*cp); surfaceScalarField rhoPhiCp("rhoPhiCp", rhoPhi*fvc::interpolate(cp)); fvScalarMatrix hEqn ( fvm::ddt(rhoCp, T) + fvm::div(rhoPhiCp, T) - fvm::laplacian(lambda, T) ); solve ( hEqn == - hs*fvc::ddt(rho, gamma) //Source term from Stefan condition ); The source term derived from the Stefan condition takes care of the temperature gradient at the interface induced by the phase change. Solver: Like in interFoam, the solver works as follows: Solving gamma equation Solving coupled pressure and velocity equations NEW solving energy equation NEW The solver is very unstable what, in my opinion is due to the couppling of gamma and energy. Please correct me when I am wrong. My questions are: Is it really the coupling of gamma and energy, making the solver instable? Is there a way to solve the coupled equations (relaxation)? Thanks allot for your replies. Best regards Fabian

 May 18, 2009, 09:51 Simulation stops #2 Senior Member     Fabian Roesler Join Date: Mar 2009 Location: Bad Friedrichshall, Germany Posts: 161 Rep Power: 8 Hallo Foamers I managed to get my model running. I substituted the gamma equation into the energy conservation equation and it worked. No I encountered another problem. The solver runs fine until a certain time, where all iteration numbers equal zero and the results do not change anymore. The solver continues running until endTime but nothing changes anymore. Here are the two time steps from the log file where the error occurred in between: PBiCG: Solving for T, Initial residual = 1.00244e-05, Final residual = 8.71675e-11, No Iterations 1 Liquid phase volume fraction = 0.00105084 Min(gamma) = 0.000769482 Max(gamma) = 0.998571 PBiCG: Solving for Ux, Initial residual = 0.000224831, Final residual = 1.0262e-16, No Iterations 1 PBiCG: Solving for Uy, Initial residual = 0.000162936, Final residual = 7.40847e-17, No Iterations 1 PCG: Solving for pd, Initial residual = 0.000982493, Final residual = 1.25233e-05, No Iterations 2 PCG: Solving for pd, Initial residual = 1.25111e-05, Final residual = 4.69217e-07, No Iterations 23 PCG: Solving for pd, Initial residual = 4.69216e-07, Final residual = 7.52164e-08, No Iterations 25 PCG: Solving for pd, Initial residual = 7.55978e-08, Final residual = 7.55978e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55978e-08, Final residual = 7.55978e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55978e-08, Final residual = 7.55978e-08, No Iterations 0 time step continuity errors : sum local = 2.05188e-15, global = 1.44131e-30, cumulative = -4.99715e-30 ExecutionTime = 287.72 s ClockTime = 288 s Courant Number mean: 2.76148e-12 max: 7.1681e-10 velocity magnitude: 2.51386e-11 deltaT = 0.00990099 Time = 11.7822 PBiCG: Solving for T, Initial residual = 9.99292e-06, Final residual = 9.99292e-06, No Iterations 0 Liquid phase volume fraction = 0.00105084 Min(gamma) = 0.000769482 Max(gamma) = 0.998571 PBiCG: Solving for Ux, Initial residual = 1.10625e-12, Final residual = 1.10625e-12, No Iterations 0 PBiCG: Solving for Uy, Initial residual = 6.0714e-13, Final residual = 6.0714e-13, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55979e-08, Final residual = 7.55979e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55979e-08, Final residual = 7.55979e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55979e-08, Final residual = 7.55979e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55979e-08, Final residual = 7.55979e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55979e-08, Final residual = 7.55979e-08, No Iterations 0 PCG: Solving for pd, Initial residual = 7.55979e-08, Final residual = 7.55979e-08, No Iterations 0 time step continuity errors : sum local = 2.05188e-15, global = -4.11243e-31, cumulative = -5.40839e-30 ExecutionTime = 287.81 s ClockTime = 288 s Courant Number mean: 2.76148e-12 max: 7.16811e-10 velocity magnitude: 2.51386e-11 deltaT = 0.00990099 Time = 11.7921 I think all residuals are OK and the Courant number is way to small to have an effect. Any ideas what could cause this problem? Thanks in advance for your replies. Regards

 June 2, 2009, 12:00 #3 Member   Rachel Vogl Join Date: Jun 2009 Posts: 48 Rep Power: 8 Hi Fabian, My guess is that the reducing the number of pd iterations might solve the issue. I guess its the non-orthogonal pressure corrections. In case this does not work, consider reducing the residual to say e-10 or relTol parameters. Regards Rachel

 June 3, 2009, 03:37 PISO in multiphase phase change problems #4 Senior Member     Fabian Roesler Join Date: Mar 2009 Location: Bad Friedrichshall, Germany Posts: 161 Rep Power: 8 Hi Rachel Thank you for your reply. You are right: It's the residual causing this problem. The initial residual PBiCG: Solving for T, Initial residual = 9.99292e-06, Final residual = 9.99292e-06, No Iterations 0 is allready below the one beeing requested by fvSolution. I set the residual to 1e-10 and the simulation runs without problems. However I have still some problems with continuity. Like in the cavitation multiphase solvers, the PISO pressure equation has to be changed in a certain way. In interPhaseChange Foam for example, pEqn is changed from fvScalarMatrix pdEqn ( fvc::div(phi) - fvm::laplacian(rUAf, pd) ); to fvScalarMatrix pdEqn ( fvc::div(phi) - fvm::laplacian(rUAf, pd) + (vDotvP - vDotcP)*(rho*gh - pSat) + fvm::Sp(vDotvP - vDotcP, pd) ); I have to have a closer look on the PISO scheme and the pressure equation to learn how to derive the equation suited to my model. Does anybody have some tips on how to use PISO in phase change multiphase problems? Thanks allot in advance. Regards Fabian

 June 4, 2009, 10:53 substitution of equation into the energy conservation equation #5 Member   Hamed Aghajani Join Date: Mar 2009 Location: London, UK Posts: 77 Rep Power: 8 Dear Fabian, Would you please let me know, how do you substituted the gamma equation into the energy conservation equation. Please drop some lines, how this could solve the problem arose? Thanks in advance, Hamed

 June 5, 2009, 06:18 #6 New Member   Join Date: May 2009 Posts: 7 Rep Power: 8 Hi Fabian, I'm also interested in solidification simulation, but i have some problems in defining gamma as a function of temperature. Can you tell me how you did? Dario

 June 5, 2009, 06:45 Continuous gamma function #7 Senior Member     Fabian Roesler Join Date: Mar 2009 Location: Bad Friedrichshall, Germany Posts: 161 Rep Power: 8 Hi Hamed, hi Dario My gamma equation is in contrast to the literature a continuous function. The literature defines gamma as 0 in the solid phase, 1 in the liquid phase and linear in between. I am using a arcus tangent function. dimensionedScalar alpha = (Tl-Ts)/(scalar(2)*tan(scalar(0.49)*pi)); gamma = atan(scalar(1)/alpha*(T-(Tl+Ts)/scalar(2)))/pi+scalar(0.5); The source term in the energy equation - hs*fvc::ddt(rho, gamma) can be written as - hs* ( rho*fvc::ddt(gamma) + gamma*fvc::ddt(rho) ); the time derivative of gamma can be directly included here so the two coupled equations form one equation. The gamma field can be calculated after solving the energy equation, however this is not necessary for the solver any more. Anybody can tell me more about the PISO scheme in multiphase solvers? Regards Fabian

May 27, 2010, 10:11
#8
Member

Jitao Liu
Join Date: Mar 2009
Location: Jinan , China
Posts: 64
Rep Power: 8
Quote:
 Originally Posted by fabian_roesler Hi Hamed, hi Dario My gamma equation is in contrast to the literature a continuous function. The literature defines gamma as 0 in the solid phase, 1 in the liquid phase and linear in between. I am using a arcus tangent function. dimensionedScalar alpha = (Tl-Ts)/(scalar(2)*tan(scalar(0.49)*pi)); gamma = atan(scalar(1)/alpha*(T-(Tl+Ts)/scalar(2)))/pi+scalar(0.5); The source term in the energy equation - hs*fvc::ddt(rho, gamma) can be written as - hs* ( rho*fvc::ddt(gamma) + gamma*fvc::ddt(rho) ); the time derivative of gamma can be directly included here so the two coupled equations form one equation. The gamma field can be calculated after solving the energy equation, however this is not necessary for the solver any more. Anybody can tell me more about the PISO scheme in multiphase solvers? Regards Fabian

Hi Fabian,

I am trying to simulate melt filling process in injcetion molding. The polymer melt solidifies and stops flowing at cavity wall due to the cooling effect of cold cavity. As a result, the melt/air and melt/solid interfaces need to be fixed in simulation. I have added the energy equation into interFoam. The non-newtonian viscosity is take into account, too. The problem is that how can I determine the varied melt/solid interface.

Best regards,
Jitao

 May 28, 2010, 08:45 Gamma function for injection molding #9 Senior Member     Fabian Roesler Join Date: Mar 2009 Location: Bad Friedrichshall, Germany Posts: 161 Rep Power: 8 Hi Jitao the phase change is taken into account by adding a source term to the energy conservation equation. Internal energy is no longer cp*T but cp*T + gamma*hs where gamma is the phase fraction and hs is the latent heat of fusion. The method is called the enthalpy method. It can be used when phase change occurs over a temperature range and without crystallisation effect. Regards Fabian

September 1, 2010, 18:01
#10
Member

Join Date: Nov 2009
Posts: 48
Rep Power: 7
Hi Fabian,

First of all Thank you for sharing your information. Second, I have some question regarding the solidification (Ice accretion ) with interFoam.
1- does your mesh update in each iteration?
2- have you managed to get good result?
3- can you explain it to how does it works, I mean I did not see any condition in your solid -liquid phase for temperature. I guess you involve the condition in your gamma, am I right??
Finally would you please give me some hint or any progress in your implementation?

Thanks

Mehran

Quote:
 Originally Posted by fabian_roesler Hi Jitao the phase change is taken into account by adding a source term to the energy conservation equation. Internal energy is no longer cp*T but cp*T + gamma*hs where gamma is the phase fraction and hs is the latent heat of fusion. The method is called the enthalpy method. It can be used when phase change occurs over a temperature range and without crystallisation effect. Regards Fabian

 December 24, 2012, 07:37 #11 New Member   mamadreza Join Date: Mar 2011 Posts: 22 Rep Power: 6 hi Have you succeeded in solidification in OpenFoam? I am facing a similar problem and I want to model the aircraft in-fight ice accretion using openfoam or fluent please help me about this problem ThankS

 Tags coupling, interfoam, phase change, piso, solid/liquid

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Piti CFX 0 February 9, 2009 10:27 Ahmad Al-Zoubi CFX 1 November 26, 2008 04:59 ohrmond CFX 2 May 26, 2006 06:27 CFDflying CFX 1 February 18, 2004 05:10 youngan CFX 0 July 1, 2003 23:32

All times are GMT -4. The time now is 04:41.