CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Viscoelastic Fluid Flows using OpenFOAM The solver viscoelasticFluidFoam

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

Like Tree23Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 22, 2009, 14:25
Default
  #41
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   May 27, 2009, 12:03
Default
  #42
Member
 
xianghong wu
Join Date: Mar 2009
Posts: 57
Rep Power: 8
wendywu is on a distinguished road
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
File Type: doc how to solve viscoplastic contitutive problem.doc (46.5 KB, 244 views)
wendywu is offline   Reply With Quote

Old   May 27, 2009, 12:09
Default
  #43
New Member
 
Jean-Luc Pelerin
Join Date: Mar 2009
Posts: 21
Rep Power: 8
jlpelerin is on a distinguished road
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
jlpelerin is offline   Reply With Quote

Old   May 27, 2009, 12:13
Default
  #44
Member
 
xianghong wu
Join Date: Mar 2009
Posts: 57
Rep Power: 8
wendywu is on a distinguished road
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
wendywu is offline   Reply With Quote

Old   July 20, 2009, 08:45
Default
  #45
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   August 11, 2009, 04:48
Default
  #46
Member
 
Join Date: Jul 2009
Posts: 63
Rep Power: 8
anon_c is on a distinguished road
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
anon_c is offline   Reply With Quote

Old   August 12, 2009, 17:51
Default
  #47
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   August 15, 2009, 13:22
Default ViscoElastic in OF 1.6
  #48
New Member
 
Ray
Join Date: Aug 2009
Posts: 2
Rep Power: 0
RayExt is on a distinguished road
Is it possible to run the viscoelastic solver in OF 1.6?
RayExt is offline   Reply With Quote

Old   August 17, 2009, 12:28
Default
  #49
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   August 18, 2009, 07:51
Question viscoelasticFluidFoam
  #50
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
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
ata is offline   Reply With Quote

Old   August 18, 2009, 09:27
Default
  #51
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   August 26, 2009, 06:52
Default
  #52
Member
 
Join Date: Jul 2009
Posts: 63
Rep Power: 8
anon_c is on a distinguished road
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
anon_c is offline   Reply With Quote

Old   September 10, 2009, 13:47
Default
  #53
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   September 10, 2009, 14:41
Default
  #54
Member
 
Join Date: Jul 2009
Posts: 63
Rep Power: 8
anon_c is on a distinguished road
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
anon_c is offline   Reply With Quote

Old   September 11, 2009, 02:31
Default Two Phase Viscoelastic Fluid Flow
  #55
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
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
ata is offline   Reply With Quote

Old   September 14, 2009, 09:21
Default
  #56
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Old   September 15, 2009, 03:19
Default Two Phase Viscoelastic Fluid Flow
  #57
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 8
ata is on a distinguished road
Hello Jovani
Thanks
Good luck

Ata
ata is offline   Reply With Quote

Old   September 16, 2009, 04:46
Default ViscoElasticFluid Foam In parallel
  #58
New Member
 
Prashobh
Join Date: Sep 2009
Posts: 1
Rep Power: 0
Prashobh is on a distinguished road
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
Prashobh is offline   Reply With Quote

Old   September 18, 2009, 13:28
Default problems in installing the viscoelasticFluidFoam solver in OpenFOAM 1.6
  #59
New Member
 
Teresa Margarida Mata
Join Date: Sep 2009
Posts: 3
Rep Power: 7
tmata2002 is on a distinguished road
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<double>::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<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> 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
tmata2002 is offline   Reply With Quote

Old   September 18, 2009, 16:55
Default
  #60
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 9
jovani is on a distinguished road
Send a message via Skype™ to jovani
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
jovani is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
VOF simulation of a viscoelastic fluid sinah OpenFOAM Running, Solving & CFD 10 November 25, 2010 12:02
FREE SURFACE VISCOELASTIC FLOWS Valdemir G. Ferreira Main CFD Forum 6 December 18, 2009 07:14
Viscoelastic flow modeling in OpenFOAM vulda OpenFOAM Running, Solving & CFD 1 March 17, 2008 08:32
Polyflow & OpenFoam on Viscoelastic flow modeling Sumeshen Main CFD Forum 0 March 14, 2008 09:29
Viscoelastic fluid codes joel davison Main CFD Forum 0 November 6, 2001 06:09


All times are GMT -4. The time now is 13:57.