
[Sponsors] 
August 5, 2014, 09:56 

#161 
Senior Member
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 210
Rep Power: 11 
Hi
Soon, there will be my PhD thesis available. I am in the final state of printing and it will also be available as eBook. I will post the link here. Moreover, my former colleges from the chair of engineering thermodynamics and transport processes (LTTT) at the University of Bayreuth an I prepare a new article. Cheers Fabian 

August 5, 2014, 10:39 

#162 
Member
YS
Join Date: Jan 2010
Posts: 79
Rep Power: 9 
Hi Fabian
I did a quick test today and the short conclusion is that the convMeltFoam, which uses inner iterations to update alpha, gives different result to erfConvectionMeltFoam,which uses continuous alpha function. The plots given in my earlier thread were due to the former solver and the later solver gives result sort of similar to what you presented in your paper. 

August 5, 2014, 13:18 

#163 
New Member
Akash
Join Date: Jun 2014
Location: Oslo
Posts: 29
Rep Power: 4 
@fabian
Sure, would be happy to read your thesis. Kindly post it here when you are done with it. @YS Can I have access to the paper you are referring to? Cheers 

August 6, 2014, 22:20 

#164 
Member
YS
Join Date: Jan 2010
Posts: 79
Rep Power: 9 
Hi Fabian,
I have attached two cases below, galliumErfMelting and LHTES, and they are exactly prepared according to your 2011 paper. I am using erfConvectiveMeltingPimpleFoam on OpenFOAM 2.1.1. The validation on galliumErfMelting is perfect but the result of the other case, LHTES, is somehow weird. After 10h of simulation time (36000 sec), the wax is hardly melting. Please help to have a quick look to see if there's anything I missed. Thanks a lot for the help! erfConvectiveMeltingPimpleFoam_OF210.tar.gz galliumErfMelting.tar.gz LHTES.tar.gz I tried to replace the wax by gallium in the LHTES case and the material is melting normally. Last edited by Ya_Squall2010; August 7, 2014 at 21:24. 

August 8, 2014, 10:30 
convMeltFoam Problem

#165 
New Member
P Buck
Join Date: Aug 2014
Posts: 2
Rep Power: 0 
Dear Folks,
for my MasterThesis i want to simulate the partial melting of a moving plate (quadratic) under a stationary heat source (laserwelding). I successfully downloaded and compiled the convMeltFoam  Solver for OF 2.3. For a nonmoving solid region everything works just perfect. But when i added the modifications to the solver which has been posted to simulate a moving solid region the Temperaturedistribution doesn't change and the pressure rises rapidly. Also the simulation crashes after a few timesteps. Modifications in createFields.H Code:
volVectorField Us ( IOobject ( "Us", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); Code:
fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U)  fvm::laplacian(nu, U) + fvm::Sp(DC/rho, U)  DC*Us/rho ); UEqn.relax(); My boundarys are: U Code:
internalField uniform ( 0 0 0 ); boundaryField { ground // This is actually the top of the plate where the heat source // is supplied { type slip; } maxZ { type fixedValue; value uniform ( 0 0 0 ); } minX { type fixedValue; value uniform ( 0 0 0 ); } maxX { type fixedValue; value uniform ( 0 0 0 ); } minY { type fixedValue; value uniform ( 0 0 0 ); } maxY { type fixedValue; value uniform ( 0 0 0 ); } Code:
internalField uniform ( 0 0.1667 0 ); boundaryField { ground { type slip; } maxZ { type fixedValue; value uniform ( 0 0.1667 0 ); } minX { type fixedValue; value uniform ( 0 0.1667 0 ); } maxX { type fixedValue; value uniform ( 0 0.1667 0 ); } minY { type fixedValue; value uniform ( 0 0.1667 0 ); } maxY { type zeroGradient; } Code:
internalField uniform 0; boundaryField { ground { type fixedFluxPressure; rho rhok; value uniform 0; } maxZ { type fixedFluxPressure; rho rhok; value uniform 0; } minX { type fixedFluxPressure; rho rhok; value uniform 0; } maxX { type fixedFluxPressure; rho rhok; value uniform 0; } minY { type fixedFluxPressure; rho rhok; value uniform 0; } maxY { type fixedFluxPressure; rho rhok; value uniform 0; } Thanks in advance for any help. Best Phil 

August 19, 2014, 02:40 

#166 
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 713
Rep Power: 15 
@Anja Miehe: Thanks for the solver. I have OF2.3.0 and while compiling the solver I get following warnings:
Code:
/opt/openfoam230/src/finiteVolume/lnInclude/readTimeControls.H:38:8: warning: unused variable ‘maxDeltaT’ [Wunusedvariable] readControls.H:4:9: warning: unused variable ‘minTCorr’ [Wunusedvariable] readControls.H:5:9: warning: unused variable ‘maxTCorr’ [Wunusedvariable] readControls.H:6:12: warning: unused variable ‘alphaTol’ [Wunusedvariable] readControls.H:7:12: warning: unused variable ‘alphaRel’ [Wunusedvariable] Do you think these warnings are serious? If so how can I modify the solver code to avoid them? 

August 19, 2014, 02:55 
warning: unused variable

#167 
Senior Member
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 210
Rep Power: 11 
Hi,
those warnings appear because of the curly brackets around the TEqn. The variables are defined outside these brackets and are only used inside. Thus, the compiler does not recognized their usage. So everything is fine. @ Phil: I need some time to study your problem Cheers Fabian 

August 19, 2014, 03:39 

#168 
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 713
Rep Power: 15 
@fabian_roesler: Thank you for the prompt reply.


August 19, 2014, 09:28 

#169 
New Member
P Buck
Join Date: Aug 2014
Posts: 2
Rep Power: 0 
Hy Fabian,
i did proceed with my problem. The key was to deactivate the MomentumPredictor and to use uncorrected divschemes. Furthermore it is necessary to define the inlet and outlet velocity boundaries in the UFile. Only the internal field values from Us are needed. Now the temperature distribution looks way better and the velocity magnitude (flow of the molten metal around a keyhole (capillary) in the middle of the plate ) looks more realistic than before. (See attached picture) Nevertheless the pressure distribution looks quite unrealistic. I would expect a pressure rise in front of the capillary to force the fluid around the capillary. P.S. The metal is completely fluent in the capillary region, thus a collision with the soild is not the problem. P.S.2 If i change the inlet velocity boundary to fixedValue, everything explodes. Best Phil 

August 20, 2014, 07:07 

#170 
New Member
Akash
Join Date: Jun 2014
Location: Oslo
Posts: 29
Rep Power: 4 
Hullo Fabian
I have conducted some test runs and compared with the experimental data available as a part of my master thesis. It was interesting to note that once the solid melted, a lot of noise in the temperature can be observed. I am not really sure if its numerical or physical. I checked for an other probe at a different location where the solid has not melted yet. Here no oscillations can be observed. Can you have a look at the plots I attached and kindly comment on it? Cheers 

August 26, 2014, 00:24 

#171 
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 132
Rep Power: 7 
Hi Akash,
Have you checked with the fined mesh ? cheers shakil 

August 27, 2014, 03:03 

#172  
Senior Member
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 210
Rep Power: 11 
Hi
Quote:
Quote:
Cheers Fabian 

August 27, 2014, 04:05 

#173 
New Member
Akash
Join Date: Jun 2014
Location: Oslo
Posts: 29
Rep Power: 4 
Hi Ahmed
The mesh is fine but not finest. I did a grid study for my geometry and I took mesh levels of 0.5, 1 and 2 million. There is a noticeable difference from half to one million. But one to two million has little change. Considering the computational resources available to me, I opted for 1 million cells which looked like an optimum solution. Maybe taking 2 million cells will dampen the oscillitations but I am not sure if they will eliminate them entirely. What do you think? Cheers Akash 

August 27, 2014, 04:16 

#174 
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 6 
Hi Akash
From the plots attached, after the melting point of the solid. The solver tends to be chaotic due to the modeling of convection. Which algorithm are you using the one with error function or an iterative approach? Best Regards Rohith 

August 27, 2014, 05:26 

#175 
New Member
Akash
Join Date: Jun 2014
Location: Oslo
Posts: 29
Rep Power: 4 
Hi Rohith
The solver I am using is convMeltFoam from Fabian. Could you be more specific about what you mean by the algorithm employed? You mean the pressure corrector or something else? Cheers Akash 

August 27, 2014, 05:40 

#176 
Member
Rohith
Join Date: Oct 2012
Location: Germany
Posts: 57
Rep Power: 6 
Hi Akash
The algorithm, i mentioned means the approach used to model the temperature and Enthalpy coupling. However, i see that you have used ConvMeltFoam which means the temperature follows source based iterative approach by Voller et al., i may suggest you to reduce the time step size as well with different mesh refinements to optimize the courant number. The oscillations you mentioned above could be possible due to the iterations. But it seems a bit strange to me that the slope and curvature vary very large from the experimental results. My call would be try to make the approximation more stiff in modeling temperature. Regards Rohith 

August 27, 2014, 07:59 

#177 
New Member
Akash
Join Date: Jun 2014
Location: Oslo
Posts: 29
Rep Power: 4 
Hi Rohith
Thank you for the suggestions. I would try to implement them and see how it goes. As you indicated, the slopes are quite different but after having a word with the testing department we have come to conclusion that the experimental values are also error prone. Especially probe 2(the first picture) as it is located between the heaters (my geometry has two parallel heaters in a tank). It was quite difficult to measure with reasonable accuracy. But probe 17(second picture) is far away from the heaters and shows good relation with experimental values. Nonetheless, it would be interesting to see what would happen with probe 17 once melting front reaches the location. I have not yet run that far. Cheers Akash 

October 6, 2014, 10:51 

#178 
Senior Member
anonymous
Join Date: Aug 2014
Posts: 199
Rep Power: 4 
Hi guys,
I´m having some doubts about how to implement the source terms in Openfoam. Currently there seems to be two approaches: 1) Fabian Rösler's one, based on writing the enthalpy equation in terms of the liquid fraction writing the terms which depends on the liquid fraction as explicit ( fvc:: ) 2) Voller's approach, based on linearized source terms as follows: Whith both of them correcting the liquid fraction after each iteration So which one would the best one to implement? I mean, Voller didn´t take account of convection, so the convection source term doesn´t appear in his equations. But Voller´s method has been validated in numerous testcases. Also I've validated Rösler approach in easygeometry testcases, but I didn´t use it in complexgeometries. Thank you all for the cooperation 

October 6, 2014, 20:28 

#179 
Senior Member
Mohammad Shakil Ahmmed
Join Date: Oct 2012
Location: AUS
Posts: 132
Rep Power: 7 
Hi anonymous,
First of all, both of the methods are good. But for the implementation it depends on what type of problem you are solving. Linearised Source Based Method (LSM) is robust, and it just takes (at least) 34 iteration for convergence. Second method, which called Fictitious Source Method (FSM), takes a little bit more iteration to converge. Now for the use, it depends on how the thermal gradient is changing. If thermal gradient changes strongly with times, then LSM may give some false results for the melt front and you may observe some false diffusion. In this case, my personal observation, it is better to go with FSM. Another problem for the LSM is to get the convergence of the results. Also, none of the method is good for isothermal phase change. If thermophysical properties are function of temperature, then LSM will cause problem unless careful steps are not taken. cheers, #shakil 

October 8, 2014, 07:15 
PhD Thesis on modeling and simulation of phase change processes in macro encapsula

#180 
Senior Member
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 210
Rep Power: 11 
Hi Folks
My PhD thesis on modeling and simulation of phase change processes in macro encapsulated latent heat thermal energy storage is now published. It is written in German and was published by the Logos Verlag Berlin. Modellierung und Simulation der Phasenwechselvorgänge in makroverkapselten latenten thermischen Speichern Thermodynamik: Energie  Umwelt  Technik, Bd. 24 Fabian Rösler ISBN 9783832537876 http://www.logosverlag.de/cgibin/e...87&lng=deu&id= The convMeltFoam solver as well as the solver which takes unconstrained close contact melting and an additional gas phase into account are explained in detail. Experimental validation in an rectangular cavity is performed. Hope you like it. Cheers Fabian 

Tags 
melting openfoam 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Melting and solidification with free surface problem?  cqlwj123  CFX  6  July 25, 2013 02:46 
Can I solve this problem by Fluent?  Kai_kc  FLUENT  1  October 27, 2010 05:29 
natural convection problem for a CHT problem  SeHee  CFX  2  June 10, 2007 06:29 
Adiabatic and Rotating wall (Convection problem)  ParodDav  CFX  5  April 29, 2007 19:13 
Melting Problem  M  FLUENT  0  April 29, 2007 16:07 