
[Sponsors] 
June 2, 2009, 14:05 

#41 
Member

@ Rachel,
As the simulation was not stable I tried using first order schemes for all variables and I changed the pressure tolerance to 1 e04 Can I mail you the case setup files because I had some problems in attaching .rar files here in the forum @ Alberto, I am trying to simulate ladlecasting where Argon will be injected to the molten steel at the bottom. As you said, the ratio of densities where too high I tried to increase the discrete phase density for stable simulation but I don't know how it will influence the flow physics.. Regards Raghavendra 

June 2, 2009, 16:44 

#42 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi,
increasing the tolerance on pressure is not going to help. It will make the code run a bit faster at the beginning, but you actually want to reduce that tolerance not to propagate errors. About your application, I have to say I do not know much about the kind of system you are considering, however did you check if there are already works done using twofluid models for that kind of application? My feeling is that it might not be the best approach. I saw casting simulations done mainly with VOF. Best, A.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 2, 2009, 18:26 

#43 
Member

Hi Alberto,
I have few results done in CFX to validate my steelargon case and it is based on twofluid approach also few literature where where steel argon simulation is performed based on two fluid modeling approach. Finally my task is to compare results what I obtained in CFX and OF. 

June 2, 2009, 18:54 

#44 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi,
could you point me to those references? I'm interested in taking a look at them. Is the melted steel newtonian? Btw, I'm also interested in the comparison, so if you want and can stay in touch with me about that, I would be very grateful :) Best, A.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 3, 2009, 03:27 

#45 
Member
Rachel Vogl
Join Date: Jun 2009
Posts: 48
Rep Power: 8 
Good Morning Raghavendra,
I guess one problem with your case is that alpha is ve and going more than 1. Using a limiting scheme divScheme might solve the problem (it bounds variables between 0 and 1) which I suspect is that case with alpha. I will try to find more about such schemes or if you find more pl update 

June 3, 2009, 04:40 

#46 
Member

Hi Alberto,
Literatures what I am refering .. 1. Turbulent Flow of Liquid Steel and Argon Bubbles in SlideGate Tundish Nozzles: Part I. Model Development and Validation by HUA BAI and BRIAN G. THOMAS 2. Mathematical simulation of fluid flow in gasstirred liquid systems by Lifeng Zhang Taniguchi Laboratory, Department of Metallurgy, Graduate School of Engineering, Tohoku University, Aobaku, Sendai 9808579, Japan Please check your mail, I have attached these to literatures yes, I am eager to discuss the comparision results with you for steelargon Regards Raghavendra 

June 3, 2009, 04:49 

#47 
Member

Hi Rachel Vogl, Good morning
I used limiting scheme divScheme as you suggested but there was not much improvement (simulation still crashing for high density case and with free surface) Also I increased nNonOrthogonalCorrectors to 8 as my mesh is not structured but still not much success Regards Raghavendra 

June 3, 2009, 05:34 
@ Alberto

#48 
Member

I am modelling steel as Newtonian fluid


June 15, 2009, 10:29 
is that because of unstructured grid?

#49 
Member

Hi Alberto and Rachel,
I tried injecting SteelArgon with my earlier becker 3D case (rectangular bubblecolumn which I used to validate waterair case) and with some modification with pressure scheme the simulation was quite stable and also results seems to be quite good.. But with the same case setup (I mean with 0, constant and system) I tried with the cylindrical bubble column of unstructured grid (around 0.5 million cells) simulation is stable without turbulence being on. When I switch on the turbulence simulation crashes after few iterations this time because of the divergence in timestep continuity error. the residual for timestep continuity error keeps on increasing as soon as I switch on turbulence and it explodes after few iterations. Is that because of unstructured grid ? I tried increasing nonorthogonal correctors to 8 but the change what I noticed is the simulation crashes after performing few more iterations.. also I tried with nonorthogonal correctors 20 and the simulation runs for few more iterations and crashes again and again the reason for instability is that timestep continuity error residual. Regards Raghavendra 

June 16, 2009, 02:15 

#50 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi,
no, it's not the unstructured grid. If the grid is so bad to lead to instabilities you would notice it also in the laminar case. We talked some time ago about stability problems with the turbulence model in twoPhaseEulerFoam. The problem is probably the same. Btw, are you using that turbulence model with the airsteel system? P.S. What changes did you do to the pressure scheme, if you can share? Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 16, 2009, 03:41 

#51 
Member

Hi Alberto,
yes for the rectangular bubble column I used turbulence for steelair also but for the cylindrical case it is creating problem.. I changed the solver schemes for pressure p PCG { preconditioner DIC; tolerance 1e10; relTol 0; }; and used first order (upwind) schemes for k, epsilon and limited alpha between 0 to 1 by Gauss limitedLinear01 1 these are the only changes I made and it worked fine for Steelair in rectangular bubble column .. Regards Raghavendra 

June 17, 2009, 10:20 

#52 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi,
thanks for your reply. I have some doubt that with that difference in the fluid properties you can use the turbulence model based on the mixture. It sounds quite a strong assumption! This said, if you suspect that the difference is actually given by the mesh, and not by the BC's or the numerics, you can still generate an hexhedral mesh for a cylinder. The typical configuration used in bubble columns is to split the section (circle) in a central square and four sides, and mesh them with hex cells. Axially you should not have any problem if the geometry is a simple cylinder without lateral inlets. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 18, 2009, 03:18 

#53 
Member

Hello Alberto,
Yes you are right. I could have started with structured grids but I already had simulation running in CFX with this unstructured grids (of 0.5 Million cells) so I though to doing with the same mesh in OF also.. Now I have to try with structured grids.. Is it advisible to change pressure scheme from piso to simpleTransient in twoPhaseEulerFoam? Regards Raghavendra 

June 18, 2009, 11:50 

#54 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi,
in my experience "multphase" and "nonhex grids" are not a good match. It takes a bit more time to generate a good hex grid, but with the same number of cells the result is typically a lot better, and the convergence too. You can change the scheme from PISO to an unsteady SIMPLE, of course. This would allow you to underrelax inside each time step, and if you want to do something more refined, to check for residuals convergence and adapt the time step as a consequence. It has been on my todo list for a long time (and it's not done yet, because I'm busy with other stuff) :( Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 18, 2009, 15:36 

#55 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
It is always interesting to see someone without anything better to do than spamming. User reported.
Update: Thanks for the cleanup to the CFDOnline people! :) Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. Last edited by alberto; June 19, 2009 at 12:54. 

June 20, 2009, 15:06 

#56 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi Raghavendra,
an additional hint: check the values of k, epsilon and the turbulent viscosity ratio (nutb/nub) where you have no liquid. I quickly took a look at those, and noticed the turbulent viscosity becomes large there. It might be worth to limit the turbulent viscosity ratio (and as a consequence k) to some upper value. Best, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 20, 2009, 17:18 

#57 
Member

Hi Alberto,
Thanks for your support I will look into that.. Have a nice weekend Regards  Raghavendra 

June 20, 2009, 17:40 

#58 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
You're welcome.
I actually coded the limiter in quite a rough manner, and I also added some submodels for gasliquid flows (bubble pressure term, bubble induced turbulence, some drag correlation for contaminated water). The turbulent viscosity limiter indeed plays an important role in my test case, which is Pfleger et al. bubble column. I represented it in 2D, with 45 cm of water in a 0.2m x 0.55m domain. If you look at the zone without liquid, the turbulent viscosity tends to become extremely high. Limiting the turbulent viscosity ratio to 10^5 there (value taken by FLUENT) stabilized the solution significantly. Coding the limiter is very easy. Before correcting the effective viscosity in kEpsilon.H, simply add these lines: Code:
scalar maxNutb = max(nutb).value(); Info << "Maximum turbulent viscosity of continuous phase = " << maxNutb << endl; if (RASturbulence && (maxNutb/nub.value() > maxTurbulentViscosityRatio) && limitNuRatio) { Info << "Warning: Limiting total viscosity ratio to " << maxTurbulentViscosityRatio << endl; nutb.min(maxTurbulentViscosityRatio*nub); k = max(sqrt(nutb*epsilon/Cmu),dimensionedScalar("zero", k.dimensions(), 1.0e8)) ; }
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 23, 2009, 04:14 

#59 
Member

Hi Alberto,
limiting nutb/nub seems to be interesting even I will try that in my Pfleger bubble column case for airwater. Coming back to Steelargon case yesterday I tried with structured mesh and simulation seems to be quite stable though it is really slow (for one second it took 4 hours with 70K cells..! I am limiting Co to 0.75 so the timestep is in the order of 0.1milliseconds) I was really surprised unstructured grid (1.2Mcells) failing for a stable simulation. The same grid in CFX took less than 2 days to complete the simulation (200 seconds of simulation) Anyways, going back to strucutred grid helped me a lot in my case. I will try with limiting nutb/nub for 2D bubble column waterair case and I will keep updating about this here Regards Raghavendra 

June 23, 2009, 16:13 

#60  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 26 
Hi,
Quote:
Quote:
Best, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Burgerbs equation non constant Boundary Conditions Initial Conditions  arkangel  OpenFOAM Running, Solving & CFD  1  October 2, 2008 14:48 
Boundary conditions for turbulent boundary layer  Thomas  FLUENT  1  June 17, 2008 05:14 
boundary conditions for boundary layer flow  A. Alzoubi  CFX  0  November 3, 2007 08:11 
TwoPhaseEulerFoam and InletOutlet boundary condition  hemph  OpenFOAM Running, Solving & CFD  10  January 29, 2007 10:47 
Integral boundary conditions turbulent intensitylength boundary conditions  olesen  OpenFOAM Running, Solving & CFD  0  July 27, 2006 07:18 