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 Tree25Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 16, 2010, 09:03
Post Hi ata
  #121
Senior Member
 
Join Date: Sep 2010
Location: France
Posts: 199
Rep Power: 7
T.D. is on a distinguished road
Hi my friend,
yes indeed i did a Model and compiled it in the folder viscosityModels
but my problem is that i need to use another model for the viscosity in the same solver, in another words,
i need to use two different viscosity models in the same solver, where these two viscosityModels i shall define.
I hope you understood me better now

note:
I know that there exists the twophaseModel, but there i can't because it combines the two viscosities in one and always return it back to one "nu" or "nuEff" with certain factor something like nu=epsilon*nu1+(1-epsilon)*nu2 you see.
but me, i need to use two different seperated models for nu1 and nu2.
so always when i build one from the existing Models like i did, i am obliged to get back the viscosity under the name "nu" you see, i can't make another model and call it "nu1" or "nu2" since it was prevoiusly built in all classes as "nu" or "nuEff".

help please
and always thanks a lot

yours,

T.D.
T.D. is offline   Reply With Quote

Old   October 16, 2010, 09:15
Default
  #122
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 9
ata is on a distinguished road
Hi T.D.
I didn't understand you completely. But can you define a new viscosity model in createFields file?
Best regards

Ata
ata is offline   Reply With Quote

Old   October 16, 2010, 09:32
Post help please
  #123
Senior Member
 
Join Date: Sep 2010
Location: France
Posts: 199
Rep Power: 7
T.D. is on a distinguished road
HI,
really, can i define it in createFields file? How?
even if my "nu1" is function of another used field like temperature "T" ?

can you just give me a simple example pleaaaaaaase:
lets say i need each time i use nu1 in the solver, i need it to be called as
nu1 = 2*T +5;
how to construct and implement nu1 in the create Fields file

help please

thanks a lot for your patience
T.D. is offline   Reply With Quote

Old   October 16, 2010, 09:45
Default
  #124
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 9
ata is on a distinguished road
Hi T.D.
If you want two non-Newtonian viscosity model use:
singlePhaseTransportModel fluid1(U, phi);
But you must do some things in the source code (As I told you)
If you want a Newtonian model with two different viscosity use:
Info<< "Reading transportProperties\n" << endl;

IOdictionary transportProperties
(
IOobject
(
"transportProperties",
runTime.constant(),
mesh,
IOobject::MUST_READ,
IOobject::NO_WRITE
)
);

dimensionedScalar nu1
(
transportProperties.lookup("nu1")
);

and then calculate it in your code.

Best regards

Ata
ata is offline   Reply With Quote

Old   October 16, 2010, 09:55
Default i need two non-Newtonian..
  #125
Senior Member
 
Join Date: Sep 2010
Location: France
Posts: 199
Rep Power: 7
T.D. is on a distinguished road
Hi
yes indeed i need two non-Newtonian viscosity Models,
so for the two viscosities how should i define them, i must put
in the singlePhaseTransportModel fluid1 and fluid2 ?, and how to link back to read the two different laws, like crosspower and power (as example)? i must use like transportModel1 "crosspower", and transportModel2 "power" in the transport properties file? if so, where to define the transportModel1 and transportModel2, is it also inside the singlephaseTransportModel file?
thanks a lot my brother

Quote:
Originally Posted by ata View Post
Hi T.D.
If you want two non-Newtonian viscosity model use:
singlePhaseTransportModel fluid1(U, phi);
But you must do some things in the source code (As I told you)
If you want a Newtonian model with two different viscosity use:
Info<< "Reading transportProperties\n" << endl;

IOdictionary transportProperties
(
IOobject
(
"transportProperties",
runTime.constant(),
mesh,
IOobject::MUST_READ,
IOobject::NO_WRITE
)
);

dimensionedScalar nu1
(
transportProperties.lookup("nu1")
);

and then calculate it in your code.

Best regards

Ata
T.D. is offline   Reply With Quote

Old   October 16, 2010, 22:12
Default
  #126
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 9
ata is on a distinguished road
Hi T.D.
I think you must define two different dictionary in your code and using constructor of your models define two different viscosity model. The constructors for CrossPowerLaw is:
CrossPowerLaw
(
const word& name1,
const dictionary& viscosityProperties1,
const volVectorField& U,
const surfaceScalarField& phi
);
and for powerlaw is:
powerLaw
(
const word& name2,
const dictionary& viscosityProperties2,
const volVectorField& U,
const surfaceScalarField& phi
);
Be careful you must define two different dictionary viscosityProperties1 nad viscosityProperties2 i.e.
Good luck
Best regards

Ata
ata is offline   Reply With Quote

Old   October 17, 2010, 04:24
Default Hi
  #127
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 7
mohsenkh599 is an unknown quantity at this point
Hello
I want to employ a solver for composite materials into the viscoelasticfluidFoam but while compiling there are errors which I cannot understand completely.
the set of equations and the code I have developed are attached.

the other parameters are constants.
the Best
Attached Images
File Type: jpg 2.jpg (83.5 KB, 62 views)
Attached Files
File Type: zip ali.zip (6.7 KB, 27 views)
mohsenkh599 is offline   Reply With Quote

Old   October 17, 2010, 11:07
Default
  #128
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 10
jovani is on a distinguished road
Send a message via Skype™ to jovani
Quote:
Originally Posted by mohsenkh599 View Post
Hello
I want to employ a solver for composite materials into the viscoelasticfluidFoam but while compiling there are errors which I cannot understand completely.
the set of equations and the code I have developed are attached.

the other parameters are constants.
the Best
Hello mohsen,

Your problem is with the term [(omega . a) - (a . omega)] in equation for "a". The return of this operation is a tensorField and not a symmTensorField. Then two options to overcome this problem:

1 - Find a manner to [(omega . a) - (a . omega)] give a symmTensor. I think this is not possible, but ...
2 - Work with tensorField type. Then, "a" need to be declared as tensor field, the fvMatriz for "a" equation and all the operations that use "a" also need be of tensorField type. See also that omega=skew(L) in OF.

Best regards,
Jovani
jovani is offline   Reply With Quote

Old   October 18, 2010, 04:36
Post Hi
  #129
Senior Member
 
Join Date: Sep 2010
Location: France
Posts: 199
Rep Power: 7
T.D. is on a distinguished road
Hi ata, and all foamers, please help i am so confused
My problem is i only need to use two different viscosityModels in the same solver.so to use two different transportModels i'll define in the dictionary.
(trasportModel1 powerlaw, and transportModel2 crosspowerLaw)

i need a clear solution pleaaaaaaaaaaase with steps if possible.
thanks ata but your answer confused me, beacause i mixed all of them the trasportModel, singlephasetrosportModel and viscosityModel directories.

Anyone has a clear solution please with some steps to follow, and where to change in which files exactly, and how to call the two different viscosities inside the solver?

Help pleaaaaaaaaase

thanks a lot
T.D. is offline   Reply With Quote

Old   October 18, 2010, 04:58
Default Hi
  #130
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 7
mohsenkh599 is an unknown quantity at this point
hello Jovani,
Thank you very much for your response. I changed every symmTensor to tensor but there are some problem now. Could you possibly take a look at this file and help me.

Best Regards.
Mohsen
Attached Files
File Type: c ali.C (5.8 KB, 27 views)
mohsenkh599 is offline   Reply With Quote

Old   October 18, 2010, 12:01
Default
  #131
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 10
jovani is on a distinguished road
Send a message via Skype™ to jovani
Quote:
Originally Posted by mohsenkh599 View Post
hello Jovani,
Thank you very much for your response. I changed every symmTensor to tensor but there are some problem now. Could you possibly take a look at this file and help me.

Best Regards.
Mohsen
Hi Mohsen,

Good, now you need make it recursive back to the tree --> multiMode --> viscoelasticLaw ..... This make the other models bad to be used. You need compile only your new model, with all library tree using tensor field. A question: How important is the assymetry introduced by the anti-symetric part of deformation tensor in your model?? Is that an important term for your purposes?

Best,
Jovani
jovani is offline   Reply With Quote

Old   October 18, 2010, 12:37
Default Hi
  #132
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 7
mohsenkh599 is an unknown quantity at this point
Hello Jovani again,
Thank you again for your reply. yes I have done this and the model is compiled now. the other viscoelastic models are not included now.
I tried to run a case with this model but there is a problem which I cannot understand. I run the "viscoelasticFluidFoam" solver in the terminal and the following massage appears:

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting viscoelastic model multiMode
Selecting viscoelastic model ali
--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field taucnffirst would be more appropriate.
--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field taucfirst would be more appropriate.
--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field afirst would be more appropriate.

Starting time loop

Courant Number mean: 0 max: 0.00016
deltaT = 1.1999e-05
Time = 1.1999e-05

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 6.11821e-12, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG: Solving for p, Initial residual = 1, Final residual = 7.87121e-08, No Iterations 391
DICPCG: Solving for p, Initial residual = 3.07354e-10, Final residual = 3.07354e-10, No Iterations 0
time step continuity errors : sum local = 2.23709e-14, global = 1.82535e-17, cumulative = 1.82535e-17
Model mode 1



valueInternalCoeffs cannot be called for a calculatedFvPatchField
on patch inlet of field taufirst in file "/home/mohsen/OpenFOAM/mohsen-1.6/run/tutorials/viscoelasticFluidFoam/mohsen/0/taufirst"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::valueInternalCoeffs( const tmp<scalarField>&) const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 145.

FOAM exiting

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

And about your question, yes I should consider this term because this expression is in the model used for fiber orientation tensor.

Best wishes,
Mohsen
mohsenkh599 is offline   Reply With Quote

Old   October 19, 2010, 06:54
Default
  #133
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 10
jovani is on a distinguished road
Send a message via Skype™ to jovani
Quote:
Originally Posted by mohsenkh599 View Post
Hello Jovani again,
Thank you again for your reply. yes I have done this and the model is compiled now. the other viscoelastic models are not included now.
I tried to run a case with this model but there is a problem which I cannot understand. I run the "viscoelasticFluidFoam" solver in the terminal and the following massage appears:

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting viscoelastic model multiMode
Selecting viscoelastic model ali
--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field taucnffirst would be more appropriate.
--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field taucfirst would be more appropriate.
--> FOAM Warning :
From function GeometricField<Type, PatchField, GeoMesh>::readIfPresent()
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C at line 107
read option IOobject::MUST_READ suggests that a read constructor for field afirst would be more appropriate.

Starting time loop

Courant Number mean: 0 max: 0.00016
deltaT = 1.1999e-05
Time = 1.1999e-05

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 6.11821e-12, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG: Solving for p, Initial residual = 1, Final residual = 7.87121e-08, No Iterations 391
DICPCG: Solving for p, Initial residual = 3.07354e-10, Final residual = 3.07354e-10, No Iterations 0
time step continuity errors : sum local = 2.23709e-14, global = 1.82535e-17, cumulative = 1.82535e-17
Model mode 1



valueInternalCoeffs cannot be called for a calculatedFvPatchField
on patch inlet of field taufirst in file "/home/mohsen/OpenFOAM/mohsen-1.6/run/tutorials/viscoelasticFluidFoam/mohsen/0/taufirst"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::valueInternalCoeffs( const tmp<scalarField>&) const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 145.

FOAM exiting

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

And about your question, yes I should consider this term because this expression is in the model used for fiber orientation tensor.

Best wishes,
Mohsen
Hello Mohsen,

This seems your internal field for taufirst is wrong, you consider a nine components for internal field, now you are working with the complete stress tensor??

If it is not this the problem no idea by looking this return messaging.

Best regards,
Jovani
jovani is offline   Reply With Quote

Old   October 19, 2010, 12:10
Default
  #134
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 7
mohsenkh599 is an unknown quantity at this point
Quote:
Originally Posted by jovani View Post
Hello Mohsen,

This seems your internal field for taufirst is wrong, you consider a nine components for internal field, now you are working with the complete stress tensor??

If it is not this the problem no idea by looking this return messaging.

Best regards,
Jovani

Hello jovani,
I appreciate your help again. no I have considered nine element for the stress tensor but there is this problem yet. The taufirst in the "0" folder is as follows:

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.4.1-dev |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "/home/jovani/jovaniFoam/foamNewSolver/cases/recentCases/upwind";
case "Giesekus";
instance "0";
local "";

class volTensorField;
object taufirst;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [1 -1 -2 0 0 0 0];

internalField uniform (0 0 0 0 0 0 0 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0 0 0 0 0 0 0 0);
}
fixedWalls
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}
simetry
{
type symmetryPlane;
}
frontAndBack
{
type empty;
}
}


// ************************************************** *********************** //

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%

The Best,
Mohsen
mohsenkh599 is offline   Reply With Quote

Old   October 24, 2010, 08:31
Default
  #135
Member
 
Jovani L. Favero
Join Date: Mar 2009
Location: Rio de Janeiro, RJ, Brazil
Posts: 41
Rep Power: 10
jovani is on a distinguished road
Send a message via Skype™ to jovani
Quote:
Originally Posted by mohsenkh599 View Post
Hello jovani,
I appreciate your help again. no I have considered nine element for the stress tensor but there is this problem yet. The taufirst in the "0" folder is as follows:

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.4.1-dev |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "/home/jovani/jovaniFoam/foamNewSolver/cases/recentCases/upwind";
case "Giesekus";
instance "0";
local "";

class volTensorField;
object taufirst;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [1 -1 -2 0 0 0 0];

internalField uniform (0 0 0 0 0 0 0 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0 0 0 0 0 0 0 0);
}
fixedWalls
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}
simetry
{
type symmetryPlane;
}
frontAndBack
{
type empty;
}
}


// ************************************************** *********************** //

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%% %%%%%%

The Best,
Mohsen
Hello Mohsen,

I am not sure about the problem, but i can contribute with a tip:

try to use fully 3D geometry for your simulation, i.e, do not use the empty BC:
frontAndBack
{
type empty;
}

Best,
Jovani
jovani is offline   Reply With Quote

Old   October 27, 2010, 09:14
Default Hi
  #136
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 7
mohsenkh599 is an unknown quantity at this point
Quote:
Originally Posted by jovani View Post
Hello Mohsen,

I am not sure about the problem, but i can contribute with a tip:

try to use fully 3D geometry for your simulation, i.e, do not use the empty BC:
frontAndBack
{
type empty;
}

Best,
Jovani
Hello Jovani,
Thank you very much for your reply again. I have got that there is problem in my code and I fix it. now it works.

the Best,
Mohsen
mohsenkh599 is offline   Reply With Quote

Old   November 12, 2010, 09:42
Default Hi
  #137
Member
 
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 7
mohsenkh599 is an unknown quantity at this point
Hello,
when I run my case an error message appear that I cannot understand. could anybody help me pls? the error is as follows:

%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting composite model multiMode
Selecting composite model composite8

Starting time loop

Courant Number mean: 0 max: 2e-05
deltaT = 1.1999e-05
Time = 1.1999e-05

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.38625e-10, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG: Solving for p, Initial residual = 1, Final residual = 3.94021e-08, No Iterations 76
DICPCG: Solving for p, Initial residual = 1.91826e-10, Final residual = 1.91826e-10, No Iterations 0
time step continuity errors : sum local = 4.72796e-15, global = -2.31815e-17, cumulative = -2.31815e-17
Model mode 1


lowerPtr_ or upperPtr_ unallocated#0 Foam::error:rintStack(Foam::Ostream&) in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::Ostream& Foam:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/compositeFoam"
#3 Foam::lduMatrix::lower() const in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::lduMatrix::sumMagOffDiag(Foam::Field<double> &) const in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::fvMatrix<Foam::Tensor<double> >::relax(double) in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoTransportModels.so"
#6 Foam::composite8::correct() in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoTransportModels.so"
#7 Foam::multiMode::correct() in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoTransportModels.so"
#8 Foam::compositeModel::correct() in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libviscoTransportModels.so"
#9 main in "/home/mohsen/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/compositeFoam"
#10 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#11 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/i386/elf/start.S:122


From function lduMatrix::lower() const
in file matrices/lduMatrix/lduMatrix/lduMatrix.C at line 206.

FOAM aborting

Aborted


%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%
%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%%

Best,

Mohsen
mohsenkh599 is offline   Reply With Quote

Old   April 29, 2011, 03:00
Default
  #138
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 7
anijdon is on a distinguished road
hello M.r kamyabi;
excuse me I forced a problem with openFoam. I want to modify simpleFoam to be used for nanofluid which is mixture of base fluid and nano particle and is single phase in lower volume fraction. so I should combine this two material properties as some obtained nanofluid formulas which I'll attach here:
formulas.zip

I add some lines in creatField ana .C files of my solver which is here:

nanoalaki.zip

but there is some errors which is in the error file of last zipped file;
I don't underastand what's the problem; would you tell the mistakes?
my another quastion is that should I alter the momentom equation on base of effective properties of nanofluid?if I put for example nu instead of nuEff,Is it need to ghange?
I thank you previously;
best regards
anijdon is offline   Reply With Quote

Old   April 29, 2011, 05:47
Default Viscoelastic Fluid Flows using OpenFOAM The solver viscoelasticFluidFoam
  #139
ata
Senior Member
 
ata's Avatar
 
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 322
Rep Power: 9
ata is on a distinguished road
I think you have fundamental problems. Are you at Sharif university?
(for oral explanations)
Good luck
ata is offline   Reply With Quote

Old   April 29, 2011, 13:29
Default
  #140
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 7
anijdon is on a distinguished road
hello;
thanks for your reply; I do some correction on the createFields file but there is an error yet and it seems to be a fundamental error as you said; I'll attach it;

nano2.zip

I'm not in Tehran but if it's difficult for you to explain the problem in writing don't trouble yourself any more ;
thanks a lot;

Last edited by anijdon; April 29, 2011 at 15:01.
anijdon 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 11:23.