# Viscoelastic Fluid Flows using OpenFOAM The solver viscoelasticFluidFoam

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

 May 22, 2009, 14:25 #41 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Hello Wendy, Any observations and work to you: 1) There are some obvious implementation errors, i.e., the T is not defined, the unit for some parameters are not correct ... But forget it for this moment and lets see the model and you need search answer for 2 questions: First: obs.: etaEff=sqrt(2.0/3.0)*mag(symm(fvc::grad(U))); this is not etaEff, this is shear rate in your model! shearRate=sqrt(2.0/3.0)*mag(symm(fvc::grad(U))); and etaEff=asinh(pow(Z/A,1.0/n))/(3*beta*shearRate); Here is a good point to talk: shear rate can be zero in any place of the domain or in any cell. shearRate = 0, division by zero, etaEff-> infinity and numeric problems. What do in this case???? Who developed this model will need a solution for it, see what is it!! take a better look on all the modeling. Second: Where is D^d in momentum equation?? fvm::ddt(U) + fvm::div(phi, U) - fvm::laplacian(eta_d, U) fvm::laplacian(eta_d, U) is equal to 2*eta(D,T)D^d ?? or you need create D = symm(fvc::grad(U)) and then make 2*nuEff*dev(D) into momentum equation?? This take grad(U) explicitly into momentum equation!! Best, Jovani

May 27, 2009, 12:03
#42
Member

xianghong wu
Join Date: Mar 2009
Posts: 57
Rep Power: 10
Hi,
Jovani,

Thank you so much for your patience and time.
I have corrected my code according to your correction.
would you please check it again when you have time?
Thank you and have a nice day.

Best,
Wendy
Attached Files
 how to solve viscoplastic contitutive problem.doc (46.5 KB, 269 views)

 May 27, 2009, 12:09 #43 New Member   Jean-Luc Pelerin Join Date: Mar 2009 Posts: 21 Rep Power: 10 Hi Jovani, Congratulations! It seems like you did some great job. I am also interested in this kind of solver (for ice simulation). Do you know when you will be able to release your solver? I have tried to implement one myself but I clearly lack basic knowledge on this subject. Thank you, Regards, Jean-Luc

 May 27, 2009, 12:13 #44 Member   xianghong wu Join Date: Mar 2009 Posts: 57 Rep Power: 10 hi, Do you talk to Javani or to me? I am wendy, but I received your reply from my email box. thank you. I am a begginer and I am just learning from the beginning. we can study together anyway. Wendy

 July 20, 2009, 08:45 #45 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Hello Foamers, I want to announce the release of the solver for treatment of viscoelastic fluid flow (the viscoelasticFluidFoam solver) in the OpenFOAM-1.5-dev SVN repository. Together with the solver also was released three tools: the "PSD" tool to calculate the principal stress difference, the "stressDifferences" tool to calculate the stress differences (N1 and N2) and "stressSymmComponents" to extract the six individual components of the stress tensor tau. I think the information in the tutorial is enough to the user understand the solver (the use of all models, multimode simulation, ....), but I will be helping as far as possible users of the solver. The theory, some comments or formulation for the implemented models can be found in http://hdl.handle.net/10183/16306 where is available my master thesis (Obs.: is in Portuguese). I want to thank my advisors, Prof. Hrvoje Jasak and, Prof. Argimiro R. Secchi and Prof. Nilo S. M. Cardozo from UFRGS, for the great guidance on this work. I also want to thank Prof. Hrvoje for your code reviews. Enjoy Jovani

 August 11, 2009, 04:48 #46 Member   Join Date: Jul 2009 Posts: 63 Rep Power: 10 I just was looking for the solver and the modells and now i fiend even some tutorials very very good woork good done you have to do you phd that is very important so you can work with me on some new material modells i am just solving the tutoral of giesekus ad it take a lot of time bcz of my laptop

 August 12, 2009, 17:51 #47 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 You are rigth, is expensive for a laptop !! This is due not only because the number of cells in the mesh, but also for: in 3D geometry the stress tensor need to be solved to the 6 components and this case have 4 modes, then there are 6*4=24 equations for stress. It was to be a little expensive case Jovani

 August 15, 2009, 13:22 ViscoElastic in OF 1.6 #48 New Member   Ray Join Date: Aug 2009 Posts: 2 Rep Power: 0 Is it possible to run the viscoelastic solver in OF 1.6?

 August 17, 2009, 12:28 #49 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Yes, I PREFER the -dev version but I believe it is easy run in the 1.6 version. You need take the directory /viscoelastic (OpenFOAM-1.5-dev/src/transportModels/) and put into your OF. Add the line " wmake libso viscoelastic" in the "Allwmake" file. Now compile the library transportModels (./Allwmake). Take the solver viscoelasticFluidFoam in the OpenFOAM-1.5-dev/applications/solvers/viscoelastic/ directory. Go to the file Make/Options and remove the line " -llduSolvers" and the "\" of the line above. Then compile the solver with wmake. I do not tested it, try and post if this work. Jovani

 August 18, 2009, 07:51 viscoelasticFluidFoam #50 Senior Member     ata kamyabi Join Date: Aug 2009 Location: Kerman Posts: 323 Rep Power: 11 Hello When i try to use viscoelasticFluidFoam i confront with this error. Unknown asymmetric matrix solver BiCGStab Valid asymmetric matrix solvers are : 4 ( smoothSolver PBiCG BICCG GAMG ) Can any one help me? Thanks

 August 18, 2009, 09:27 #51 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Ok, I believe you are using a OpenFOAM version that is not the -dev version, where this problem does not exists because only in OpenFOAM -dev there is the BiCGStab solver. You need adapt all the tutorial for it. Basically you need make changes in fvSolution to change the solvers for p, U and tau. For pressure you can use PCG and for U and tau use PBiCG. Follow any other case, as for example, the fvSolution of the cavity to guide you. Jovani

 August 26, 2009, 06:52 #52 Member   Join Date: Jul 2009 Posts: 63 Rep Power: 10 hello so now i just run some cases with your models, till now every thing is ok thanks again but i have a quastin how to use interFoam with theses models is that posible?? or is it posilbe to geht the vischoelastichFoam recompiled?? did you do somthing in this direction

 September 10, 2009, 13:47 #53 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Hello, What you need is a multiphase solver with viscoelastic treatment. The viscoelasticFluidFoam solver doesn't do this, because your formulation is to closed flow of 1 only fluid. You cannot use interFoam too, because it doesn't support viscoelastic flow, only multiphase newtonian or GNF fluid. I have a solver to treat multiphase viscoelastic flow, but a can't release it now. Jovani

 September 10, 2009, 14:41 #54 Member   Join Date: Jul 2009 Posts: 63 Rep Power: 10 would you be able to relase that in the next months or you dont want to or you are not alowed to do that! i am interested on viscoelastic fluids and there mixing, i am also interested in mixing between newtoniean and nonnewtonian fluids i would be really thankful if you would be able to do something in this direction and let us know about it

 September 11, 2009, 02:31 Two Phase Viscoelastic Fluid Flow #55 Senior Member     ata kamyabi Join Date: Aug 2009 Location: Kerman Posts: 323 Rep Power: 11 Hello jovani My request is similar to tajoooko request ane i'll be glad if you answer to his questions because his questions are my questions too. Ata

 September 14, 2009, 09:21 #56 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Hello, I need to publish any paper with results of this new implementation before release. With that I can also to test better the solver and make some corrections or improvements if this is necessary. Let's say that is still under evaluation. Jovani

 September 15, 2009, 03:19 Two Phase Viscoelastic Fluid Flow #57 Senior Member     ata kamyabi Join Date: Aug 2009 Location: Kerman Posts: 323 Rep Power: 11 Hello Jovani Thanks Good luck Ata

 September 16, 2009, 04:46 ViscoElasticFluid Foam In parallel #58 New Member   Prashobh Join Date: Sep 2009 Posts: 1 Rep Power: 0 Hi Thanks for the posts, I am trying to run the viscoelasticfluidfoam example on Bluegene in parallel. I modified the case to use the PCG,PBiCG solvers, since I could not compile the lduSolvers. Are there any major performance/accuracy impacts to using PCG, PBICG solvers instead of BiCGStab? My fvSolution file looks like the following now. p PCG { preconditioner DIC tolerance 1e-07; relTol 0.0; minIter 0; maxIter 800; }; U PBiCG { preconditioner DILU minIter 0; maxIter 1000; tolerance 1e-6; relTol 0.0; }; Best Regards, Prashobh

 September 18, 2009, 13:28 problems in installing the viscoelasticFluidFoam solver in OpenFOAM 1.6 #59 New Member   Teresa Margarida Mata Join Date: Sep 2009 Posts: 3 Rep Power: 10 Hi Foamers, and in particular Jovani, I have followed the instructions given by Jovani Favero in order to install the viscoelasticFluidFoam in OpenFOAM-1.6. When I construtcted the viscoelasticTransportModels, there were some missing files errors, that I was able to solve by copying the missing files from OpenFoam-1.5-dev to OpenFOAM-1.6. I managed to compile the library. Then, I passed to the compilation of the solver itself, correcting the options file in the Make directory. The compilation started well, but I got the following errors: Making dependency list for source file viscoelasticFluidFoam.C SOURCE=viscoelasticFluidFoam.C ; g++ -m32 -Dlinux -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/transportModels/viscoelastic/lnInclude -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -IlnInclude -I. -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c \$SOURCE -o Make/linuxGccDPOpt/viscoelasticFluidFoam.o /home/titio/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readPISOControls.H: In function ‘int main(int, char**)’: /home/titio/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readPISOControls.H:8: warning: unused variable ‘momentumPredictor’ /home/titio/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readPISOControls.H:11: warning: unused variable ‘transonic’ /home/titio/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/readPISOControls.H:14: warning: unused variable ‘nOuterCorr’ g++ -m32 -Dlinux -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/transportModels/viscoelastic/lnInclude -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -IlnInclude -I. -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/home/titio/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC Make/linuxGccDPOpt/viscoelasticFluidFoam.o -L/home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt \ -lfiniteVolume -lviscoelasticTransportModels -lmeshTools -lOpenFOAM -liberty -ldl -lm -o /home/titio/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/viscoelasticFluidFoam /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::fvMatrix::solve(Foam::Istream&)' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::dictionary::lookup(Foam::word const&, bool) const' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::lduMatrix::solver::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField const&, Foam::FieldField const&, Foam::UPtrList const&, Foam::Istream&)' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::SLListBase::endIter' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::SLListBase::endConstIter' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::Ostream::writeKeyword(Foam::word const&)' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam::regIOobject::regIOobject(Foam::IOobject const&)' /home/titio/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoelasticTransportModels.so: undefined reference to `Foam:olyMesh::directions() const' collect2: ld returned 1 exit status It seems that there are errors linked to ldumatrixes and SLListBase. This means that, although the library compiled well, i have to do more things. Can anyone help me out here? Thanks in advance, Teresa Mata

 September 18, 2009, 16:55 #60 Member   Jovani L. Favero Join Date: Mar 2009 Location: Rio de Janeiro, RJ, Brazil Posts: 45 Rep Power: 11 Hello Teresa, As nobody post the results of: "You need take the directory /viscoelastic (OpenFOAM-1.5-dev/src/transportModels/) and put into your OF. Add the line " wmake libso viscoelastic" in the "Allwmake" file. Now compile the library transportModels (./Allwmake). Take the solver viscoelasticFluidFoam in the OpenFOAM-1.5-dev/applications/solvers/viscoelastic/ directory. Go to the file Make/Options and remove the line " -llduSolvers" and the "\" of the line above. " I made the test in OF1.6 in a 64 bits machine (m64) and all works fine for me. I compiled the viscoelasticTransportModels without warnings and no changes was necessary for this. Your machine is 32 bits but I think this is not the problem. After take a look in your messages I believe the problem you have to compile the solver is a problem with your libviscoelasticTransportModels.so library. Are you sure this was rigth compiled??? The directory -I\$(LIB_SRC)/transportModels/viscoelastic/lnInclude are ok?? The option of copy files from OpenFoam-1.5-dev to OpenFOAM-1.6 is not a good ideia. I think your problem is here!! You need compile the library without changes and if you cannot do it is better take a look in why do you have problems and correct this. Hello Prashobh, The changes of the solver for the linear system impact on your performance and stability and not in accuracy, this is what I know. Is like solve a problem using Bisection method and Newton Rapson method. Best, Jovani

 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 sinah OpenFOAM Running, Solving & CFD 10 November 25, 2010 12:02 Valdemir G. Ferreira Main CFD Forum 6 December 18, 2009 07:14 vulda OpenFOAM Running, Solving & CFD 1 March 17, 2008 08:32 Sumeshen Main CFD Forum 0 March 14, 2008 09:29 joel davison Main CFD Forum 0 November 6, 2001 06:09

All times are GMT -4. The time now is 23:29.