
[Sponsors] 
September 25, 2005, 13:24 
Info and Pout buffer output un

#21 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 18 
Info and Pout buffer output until an 'endl' is written.
AUTO_WRITE should work if the variable still is in scope when runTime.write() gets called. If not you can always force it to write: e.g. alpaha.write() 

September 25, 2005, 15:12 
I finally understood the probl

#22 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
I finally understood the problem.
I started to work with a version of the solver in my user directory, then I moved to the version in the OpenFOAM main directory, without removing the libraries generated by the old one. The linker still used them to link the executable, so this is the reason my changes to the code didn't take effect. I found this out by commenting out g0, and noticing that gdb still was saying me there was a floating point exception in g0. :) Now I'm doing some other test to see if the alternative g0 formulation (also adopted in MFIX) works properly. As always, thanks for your precious help. 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. 

September 30, 2005, 18:08 
Hello, what solver settings we

#23 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hello, what solver settings were used in the examples you showed me some month ago where you did the comparison between the algebraic and the differential transport equation of the granular energy?
I'm obtaining better results by approximating g0 around the packing limit and using SuperBee and limiting the gradient. My doubt is what flux do I specify for div((nuEffa*grad(Ua).T())) and div((nuEffb*grad(Ub).T())) when using an upwind scheme? Best regards, 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. 

October 3, 2005, 02:07 
Dont remember.
the divsche

#24 
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 22 
Dont remember.
the divschemes for the neff terms should be linear. 

February 6, 2006, 05:49 
1) mesh.cellCells() gives the

#25 
Super Moderator
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 18 
1) mesh.cellCells()[cellI] gives the neighbours of a cell (see primitiveMesh.H)
2) with those cell labels you can just index into any volScalarField 3) loop over all faces of a cell (mesh.cells()[cellI]) and check if any one is not an internal face (mesh.isInternalFace(faceI)) (see primitiveMesh.H) or loop over all the boundary faces and mark the owner cell (mesh.faceOwner()[faceI]). Then pick up marked cells. See User Guide about mesh ordering (boundary faces after internal faces) 

February 21, 2006, 16:52 
Hi,
1 I have a problem of co

#26 
Member
olivier Petit
Join Date: Mar 2009
Location: Göteborg, Sweden
Posts: 67
Rep Power: 10 
Hi,
1 I have a problem of convergence with twoEulerFoam. I use the different geometry and I change the schemes and time step. herewith one of my files .msh I patch the value 1 for alpha in halftop, in Inlet and in outlet in my bubble column. 0 in the halfbuttom. the diameter of Air is 0.003m the velocity in inlet is: Ua=0.0212 m/s Ub=0; I have a good result with fluent. with Foam Ur Courant Number grow up and explode. with or without turbulence. thank you for your help. 2 how can I attache my case ? 

February 21, 2006, 17:08 
To attach a file, insert the t

#27 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
To attach a file, insert the text
\ attach{Description of your file} without the space after \ The system will ask you to upload the file after you post the message. More information here: http://www.cfdonline.com/cgibin/Op...?pg=formatting Regards, 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. 

March 9, 2006, 18:48 
Hi Alberto,
I think the probl

#28 
Member
olivier Petit
Join Date: Mar 2009
Location: Göteborg, Sweden
Posts: 67
Rep Power: 10 
Hi Alberto,
I think the problem comes from the initialization of alpha (volume fraction). After the resolution of alphaequation, when alpha<0 I make it =0 and if alpha>1 I make it=1 in this case the divergence is lower. The results by fluent with the same mesh and same conditions are very good. I will add the code of population balance witch is already written for fluent (UDF) when I resolve this problem. thanks a lot for taking time to look to my case. 

March 9, 2006, 19:09 
Hi Alberto,
I think the prob

#29 
Member
olivier Petit
Join Date: Mar 2009
Location: Göteborg, Sweden
Posts: 67
Rep Power: 10 
Hi Alberto,
I think the problem comes from the initialization of alpha (volume fraction). After the resolution of alphaequation, when alpha<0 I make it =0 and if alpha>1 I make it=1 in this case the divergence is lower. The results by fluent with the same mesh and same conditions are very good. I will add the code of population balance witch is already written for fluent (UDF) when I resolve this problem. thanks a lot for taking time to look to my case. 

March 9, 2006, 20:07 
Hello Oliver,
I can't downloa

#30 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hello Oliver,
I can't download your attached file. Could you email it to me? My email address should be visible in the forum. However, the limitation of alpha between zero and one is managed in OpenFOAM by rewriting the equation for alpha in a fully conservative form, as proposed by Henry and by using a limited scheme, like limitedLinear01 or similar. Everything is well explained in the PhD thesis of Henry Rusche, downloadable from the site of Hrvoje. In my calculations, the instability is related to the kinetic theory of granular flow, because of the presence of the radial distribution function which becomes very big if the solids volume fraction gets close to the packing value. This causes instabilities in the momentum equation of the dispersed phase, due to the presence of the granular pressure gradient. I'm just testing an algorithm to avoid these problems, as I explained in another thread. Best regards, 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. 

March 24, 2006, 04:01 
Hi everyone,
I wonder how vis

#31 
New Member
Qiang Li
Join Date: Mar 2009
Location: Shenyang, LiaoNing, P. R. China
Posts: 14
Rep Power: 10 
Hi everyone,
I wonder how viscosity include bulk and collisionalkinetic distribution and pressrue of particles of kinetic theory model transfer to NS equation of solid phase in implement of twoPhaseEulerFoam. I think it is a bug! I guess this codes were originlly developed for gasliquids flow using the nature visosity of liquids in NS equation of liquids. I managed to revised the source code of UEqns.H as follows, nuEffa=kineticTheory.mua()/rhoa; volTensorField Rca = nuEffa*(fvc::grad(Ua)().T()); Rca += (2.0/3.0)*sqr(Ct)*I*k  kineticTheory.pa()/rhoa*I +kineticTheory.lambda()/rhoa*tr(fvc::grad(Ua)().T())*I  (2.0/3.0)*I*tr(Rca); Anybody tell me whether my doubt is right. What are your suggests? Thanks in advance, Best regards Q. Li 

March 24, 2006, 05:43 
Hello,
the granular pressure

#32 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Hello,
the granular pressure gradient is included in the pressure equation (pEqn.H): if (kineticTheory.on()) { phiDraga = rUaAf*fvc::snGrad(kineticTheory.pa()/rhoa)*mesh.magSf(); } You're right about the bulk viscosity, which is not included in the original solver. To keep the solver general, you can modify UEqn.H by replacing the lines: volTensorField Rca = nuEffa*(fvc::grad(Ua)().T()); Rca += (2.0/3.0)*sqr(Ct)*I*k  (2.0/3.0)*I*tr(Rca); in volTensorField gradUaT = fvc::grad(Ua)().T(); volTensorField Rca = nuEffa*gradUaT; Rca += (2.0/3.0)*sqr(Ct)*I*k  (2.0/3.0)*I*tr(Rca); if (kineticTheory.on()) { Rca += kineticTheory.lambda()/rhoa*I*tr(gradUaT); } The granular viscosity is taken into account in twoPhaseEulerFoam.C: if (kineticTheory.on()) { kineticTheory.solve(); nuEffa += kineticTheory.mua()/rhoa; } Regards, 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. 

March 24, 2006, 06:46 
Thanks for your exact and minu

#33 
New Member
Qiang Li
Join Date: Mar 2009
Location: Shenyang, LiaoNing, P. R. China
Posts: 14
Rep Power: 10 
Thanks for your exact and minute answer! I have benefited from it.
By the way, I'm also trying to simulate a bubbling bed with a jet, Schematic representation, condition and physical properties of fluidized bed come from D. J. Patil[Critical comparision of hydrodynamic models for gassolid fluidized beds part I: bubbling gassolid fluidized beds operated with a jet. Chem. Eng. Sci. 60(2005)5772]. which I used the drag model of your distribution  GidaspowErgunWenYu, viscosityModelGidaspow, conductivtyModelGidaspow. But I can't obtain a wellpleasing result. can you give me some advices! In addition I have commented codes of fictional stress model. warmly regards, Q. Li 

March 24, 2006, 08:51 
What kind of problems do you h

#34 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
What kind of problems do you have?
Can you complete the calculation, but the bubble shape is wrong? Or you can't obtain a converged solution? Regards, 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. 

March 24, 2006, 08:59 
check your Email or see follow

#35 
New Member
Qiang Li
Join Date: Mar 2009
Location: Shenyang, LiaoNing, P. R. China
Posts: 14
Rep Power: 10 
check your Email or see follows:
just as what you said on Sunday, September 18, 2005  08:19's Post "In my opinion the problems depend on the management of the packing limit. If I use the particle particle interaction force by setting g0 != 0 in the ppProperties dictionary, I get convergence, but the solid volume fraction is wrong. The bubble has a wrong form and in some case it just breaks instead of closing on itself and going up. If I set g0 = 0 in order to manage the packing limit with the kinetic theory approach, the result seems to be better, but it's impossible to complete a calculation due to convergence problems. After a few iteration I get a "nan" in the continuity equation residual. This should be related to the radial distribution function g0 which becomes infinite if the packing limit is reached. " I have encountered the same instance. Are you solve this problem? I hope you can share you experiments with me. regards Q. Li 

March 24, 2006, 09:40 
As I undertand this code has g

#36 
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 22 
As I undertand this code has gone through some improvements and if you want it included in the official 1.3 version, it might be good to send it to Henry.
Cleaned up of course. Niklas 

March 24, 2006, 10:45 
Yes. I'm working on cleaning t

#37 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Yes. I'm working on cleaning the code right now and on making a list of the changes I did.
I have some test case too which can be of interest, but I haven't extended the FoamX configuration files yet. 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. 

March 27, 2006, 19:01 
I've already implemented and g

#38 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
I've already implemented and generalised that method, which seems to work well, even though it requires a small time step (10^5).
I'm waiting for a paper acceptance and I'll release it. In the meanwhile, pay attention that the method presented in my previous post is valid only for cells of equal volume (I extended it to the general case). Also the method has to be applied not only to the packed cells but also to the neighbouring ones in order not to lose mass. Regards, 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. 

January 31, 2007, 01:41 
I wonder if twoPhaseEulerFoam

#39 
New Member
Guanghao Wu
Join Date: Mar 2009
Location: Tokyo, Japan
Posts: 15
Rep Power: 10 
I wonder if twoPhaseEulerFoam is suitable for a pipe flow with solid paticles?
I am trying to calculate the following three cases (single processor) with twoPhaseEulerFoam, and found all of the cases fell in divergence. Due to the gravity force, the solid particles will be deposited on the bottom of the pipe. So the alpha gets greater and greater and becomes alpha > 0.6~0.9 ( the value is depend on the case) . Then the solver diverges. â–*Simulation cases 3D pipe flow (liquid) with solid particles The initial conditions: alpha = 1e05 for internalField; 0.2 for inlet boundary Ua = 0m/sec for internalField; 1.0m/sec for inlet boundary Ub the same as Ua. density of liquid 900 kg/m3 density of solid particle 1100 kg/m3 â–*case 1 kineticTheory off; g0 =1, preAlphaExp=500; packingLimiter on; expMax 1.0e+03; alphaMax 0.62; â–*case 2 kineticTheory on; g0 = 0; â–*case 3 kineticTheory off; g0=0; As Alberto said, the value of alpha can not be greater than the maximum packing limit, but the kinetcTheory or particleparticle interaction model did not prevent the void fraction becoming greate than the maximum packing limit. What do you suggest? Thank you in advance. 

January 31, 2007, 04:40 
Hi Guanghao
What is your time

#40 
Senior Member
Rasmus Hemph
Join Date: Mar 2009
Location: Sweden
Posts: 108
Rep Power: 10 
Hi Guanghao
What is your time step? Packing simulations usually require a very short time step, on the order of 1e5. For your case 1, note that in OpenFOAM, the particleparticle force has the unit Pa/(kg/m^3), so your g0 should probably be divided by 1100 which might help things. Try to increase the expMax parameter to see an increase in force for an increase in alpha. //Rasmus 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Some problems with twoPhaseEulerFoam  su_junwei  OpenFOAM Running, Solving & CFD  2  November 2, 2012 02:12 
Convergence problems!!  Elleana  FLUENT  9  June 10, 2008 04:39 
Convergence problems  please help  M Liddell  FLUENT  3  February 8, 2005 20:06 
convergence problems  jeremy  FLUENT  7  May 30, 2002 06:41 
Convergence Problems  Prateep Chatterjee  FLUENT  7  October 9, 2001 09:29 