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

dynLagrangian SGS model

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 3, 2014, 14:26
Default
  #21
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 299
Rep Power: 19
Lieven will become famous soon enough
Hi vut,

Do you mean as boundary condition or initial value?
The boundary condition for walls is typically a zeroGradient...

Cheers,

L
Lieven is offline   Reply With Quote

Old   April 4, 2014, 11:46
Default
  #22
vut
Member
 
Join Date: Feb 2014
Posts: 57
Rep Power: 9
vut is on a distinguished road
Dear Lieven,

Thank you for your answer.

I am searching now the initial conditions for flm and fmm for:

- internalField
- inlet
- and outlet

Is there some formula to estimate it?

I have a turbulent inlet with fluctuation scale of 0.02 for x, y and z and a mean flow in z-direction only.

Thanks in advance,

vut
vut is offline   Reply With Quote

Old   March 30, 2016, 17:44
Default
  #23
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 15
anishtain4 is on a distinguished road
Hi,

Since there is no clear example of dynamic Lagrangian LES model in the OpenFOAM tutorials, I attached a case I had to make work.
This is for OpenFOAM 3.0.1,
Let me know if you have any questions about it.

The codes to run it are as follow:

Code:
cp -r 0.org 0;
blockMesh;
perturbUChannel;
pimpleFoam;
One also needs
Attached Files
File Type: zip dynLag.zip (11.4 KB, 241 views)
Gang Wang likes this.
anishtain4 is offline   Reply With Quote

Old   April 30, 2016, 04:18
Default
  #24
Senior Member
 
zhangyan's Avatar
 
Yan Zhang
Join Date: May 2014
Posts: 120
Rep Power: 9
zhangyan is on a distinguished road
Quote:
Originally Posted by anishtain4 View Post
Hi,

Since there is no clear example of dynamic Lagrangian LES model in the OpenFOAM tutorials, I attached a case I had to make work.
This is for OpenFOAM 3.0.1,
Let me know if you have any questions about it.

The codes to run it are as follow:

Code:
cp -r 0.org 0;
blockMesh;
perturbUChannel;
pimpleFoam;
One also needs
Hello Mahdi,
I want to know why you use the "simple filter", in your turbulenceProperties.
Because I found "laplace Filter" in the source codes, I guessed the dynLagrangian must be used accompany with "laplace Filter".

Actually, I am going to implement the dynamic K-E or dynLagrangian SGS model to another software. But I don't know how to implement the "simple Filter".

It seems that implementing laplace Filter is more easier. Could you tell me does the SGS models must be used accompany with particular Filters? For example, dynamicKEqn + simple filter; dynamicLagrangian + laplace Filter.

Another question: do you understand the simple Filter? Could you tell me the physical meaning of it?

Please forgive my poor English.

simple Filter:

tmp<volScalarField> filteredField = fvc::surfaceSum
(
mesh().magSf()*fvc::interpolate(unFilteredField)
)/fvc::surfaceSum(mesh().magSf())

laplace Filter:

tmp<volTensorField> filteredField =
unFilteredField() + fvc::laplacian(coeff_, unFilteredField())


Thanks,
Zhang Yan
zhangyan is offline   Reply With Quote

Old   October 16, 2016, 16:37
Default
  #25
Member
 
Mirage
Join Date: Jul 2012
Posts: 43
Rep Power: 11
Mirage is on a distinguished road
Hi Guys,

@Mahdi: I am also intressted to understand the meaning of ""simple filter", in your turbulenceProperties. How did u validate the accuracy of ur solver?

I would like to compare my results with a case solved with OF 2.3 and I have to make sure that I am using the same SGS model. How can I make sure that I am using the same coefficient in OF 3.0.1? Thank you .
I appreciate any help.

Last edited by Mirage; October 16, 2016 at 17:50.
Mirage is offline   Reply With Quote

Old   November 25, 2016, 06:37
Default
  #26
Member
 
Mukesh Adlak
Join Date: Jun 2016
Posts: 32
Rep Power: 7
Adlak is on a distinguished road
While running dynamicLagrangian model i am getting following error :

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[flm[0 4 -5 0 0 0 0] ] + [flm[1 1 -5 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /mnt/home/SW/CFDSupportFOAM3.0/OpenFOAM-3.0.x/src/finiteVolume/lnInclude/fvMatrix.C at line 1295.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) at ??:?
#3 Foam::tmp<Foam::fvMatrix<double> > Foam:perator+<double>(Foam::tmp<Foam::fvMatrix<d ouble> > const&, Foam::tmp<Foam::fvMatrix<double> > const&) at ??:?
#4 Foam::LESModels::dynamicLagrangian<Foam::EddyDiffu sivity<Foam::ThermalDiffusivity<Foam::Compressible TurbulenceModel<Foam::fluidThermo> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?
Aborted (core dumped)

Can anyone help me ?
Adlak is offline   Reply With Quote

Old   November 25, 2016, 07:02
Default
  #27
Member
 
Mukesh Adlak
Join Date: Jun 2016
Posts: 32
Rep Power: 7
Adlak is on a distinguished road
Quote:
Originally Posted by tidal_Tom View Post
I do not know what is causing your errors. I am a relatively novice user so it is beyond me. below are my files I used for flm and fmm. I don't think fmm can be zero, as the calculation for turbulent viscosity divides by fmm, I set this to a value of 1. flm can be zero as it is the nominator.

Have you added flm and fmm in the fvSolution and fvSchemes? lines I added are below.

fvSolution:

flm
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

fmm
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-05;
relTol 0;
}

fvSchemes:

divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,flm) Gauss limitedLinear 1;
div(phi,fmm) Gauss limitedLinear 1;
div(phi,B) Gauss limitedLinear 1;
div(B) Gauss linear;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}

and I added:

dynLagrangianCoeffs
{
filter simple;
ce 1.048;
theta 1.5;
}

in the LESProperties dictionary.

flm:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object flm;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 4 -4 0 0 0 0];

internalField uniform 0;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0;
}

outlet
{
type zeroGradient;
}

outside
{
type fixedValue;
value uniform 0;
}

object
{
type fixedValue;
value uniform 0;
}

wedge1
{
type wedge;
}

wedge2
{
type wedge;
}
}

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

fmm:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.0.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object fmm;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 4 -4 0 0 0 0];

internalField uniform 1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 1;
}

outlet
{
type zeroGradient;
}

outside
{
type zeroGradient;
}

object
{
type zeroGradient;
}

wedge1
{
type wedge;
}

wedge2
{
type wedge;
}
}

// ************************************************** *********************** //
While running dynamicLagrangian model i am getting following error :

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[flm[0 4 -5 0 0 0 0] ] + [flm[1 1 -5 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /mnt/home/SW/CFDSupportFOAM3.0/OpenFOAM-3.0.x/src/finiteVolume/lnInclude/fvMatrix.C at line 1295.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) at ??:?
#3 Foam::tmp<Foam::fvMatrix<double> > Foam:perator+<double>(Foam::tmp<Foam::fvMatrix<d ouble> > const&, Foam::tmp<Foam::fvMatrix<double> > const&) at ??:?
#4 Foam::LESModels::dynamicLagrangian<Foam::EddyDiffu sivity<Foam::ThermalDiffusivity<Foam::Compressible TurbulenceModel<Foam::fluidThermo> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?
Aborted (core dumped)

Can anyone help me ?
Adlak is offline   Reply With Quote

Old   November 28, 2016, 03:14
Default
  #28
Member
 
Mukesh Adlak
Join Date: Jun 2016
Posts: 32
Rep Power: 7
Adlak is on a distinguished road
hi everyone,

I am trying to use dynamic lagrangian les model but facing following error :

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[flm[0 4 -5 0 0 0 0] ] + [flm[1 1 -5 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /mnt/home/SW/CFDSupportFOAM3.0/OpenFOAM-3.0.x/src/finiteVolume/lnInclude/fvMatrix.C at line 1295.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) at ??:?
#3 Foam::tmp<Foam::fvMatrix<double> > Foam:perator+<double>(Foam::tmp<Foam::fvMatrix<d ouble> > const&, Foam::tmp<Foam::fvMatrix<double> > const&) at ??:?
#4 Foam::LESModels::dynamicLagrangian<Foam::EddyDiffu sivity<Foam::ThermalDiffusivity<Foam::Compressible TurbulenceModel<Foam::fluidThermo> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?
Aborted (core dumped)

If anyone can help then it will be great for me.
Thanks
Adlak is offline   Reply With Quote

Old   February 15, 2017, 11:33
Default wall function
  #29
New Member
 
bangun
Join Date: Feb 2015
Posts: 16
Rep Power: 8
eb19 is on a distinguished road
dear all,

Do we have to apply a wall function if our grid resolution near to the wall is quite coarse (let's say y+>11) even if this dynLagrangian model is applied?

In the case where wall function is necessary, do we use the standard wall function available in OpenFOAM. Please anyone give your suggestion.
eb19 is offline   Reply With Quote

Old   February 15, 2017, 12:26
Default
  #30
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 15
anishtain4 is on a distinguished road
Sorry to reply so late, have been busy past few months and missed the topic.

Q: I want to know why you use the "simple filter", in your turbulenceProperties.
A: it's the simplest model and I didn't have to worry about the filter.

Q: Could you tell me does the SGS models must be used accompany with particular Filters?
A: Theoretically now, the CFD implementation of LES should work with any form of filter or filter width, practically? the best way is to test it.

Q: do you understand the simple Filter? Could you tell me the physical meaning of it?
A: It's a tophat averaging over the filter length (usually the cell volume). This is the most common filter as it's implied by discretization, if you apply any other filter with bigger width, you are basically getting the effect of both filters. If you're going to use dynamic models then you can choose any form for the second filter as the effect of filter overlay is being considered.

Quote:
Originally Posted by zhangyan View Post
Hello Mahdi,
I want to know why you use the "simple filter", in your turbulenceProperties.
Because I found "laplace Filter" in the source codes, I guessed the dynLagrangian must be used accompany with "laplace Filter".

Actually, I am going to implement the dynamic K-E or dynLagrangian SGS model to another software. But I don't know how to implement the "simple Filter".

It seems that implementing laplace Filter is more easier. Could you tell me does the SGS models must be used accompany with particular Filters? For example, dynamicKEqn + simple filter; dynamicLagrangian + laplace Filter.

Another question: do you understand the simple Filter? Could you tell me the physical meaning of it?

Please forgive my poor English.

simple Filter:

tmp<volScalarField> filteredField = fvc::surfaceSum
(
mesh().magSf()*fvc::interpolate(unFilteredField)
)/fvc::surfaceSum(mesh().magSf())

laplace Filter:

tmp<volTensorField> filteredField =
unFilteredField() + fvc::laplacian(coeff_, unFilteredField())


Thanks,
Zhang Yan
anishtain4 is offline   Reply With Quote

Old   February 15, 2017, 12:33
Default
  #31
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 15
anishtain4 is on a distinguished road
Quote:
Originally Posted by Mirage View Post
Hi Guys,

@Mahdi: I am also intressted to understand the meaning of ""simple filter", in your turbulenceProperties. How did u validate the accuracy of ur solver?

I would like to compare my results with a case solved with OF 2.3 and I have to make sure that I am using the same SGS model. How can I make sure that I am using the same coefficient in OF 3.0.1? Thank you .
I appreciate any help.
Hi Mirage,

I solved it in a channel and the results agree well. The case is attached, you can run it.

Regarding the coefficients, the model is based on this paper:
A Lagrangian dynamic subgrid-scale model of turbulence.
(It's still the same on version 1606), so I assume the coefficients won't change as they're based on the paper.
anishtain4 is offline   Reply With Quote

Old   February 15, 2017, 12:33
Default
  #32
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 15
anishtain4 is on a distinguished road
Quote:
Originally Posted by eb19 View Post
dear all,

Do we have to apply a wall function if our grid resolution near to the wall is quite coarse (let's say y+>11) even if this dynLagrangian model is applied?

In the case where wall function is necessary, do we use the standard wall function available in OpenFOAM. Please anyone give your suggestion.
Yes and Yes.
anishtain4 is offline   Reply With Quote

Old   February 15, 2017, 13:05
Default
  #33
New Member
 
bangun
Join Date: Feb 2015
Posts: 16
Rep Power: 8
eb19 is on a distinguished road
Quote:
Originally Posted by anishtain4 View Post
Yes and Yes.
Thanks for your reply. Do you know or anyone knows if OpenFoam has a wall function which is capable for modeling flow separation? Or do you know papers that implemented this dynamic Lagrangian model for flow separation problem? Please help.
eb19 is offline   Reply With Quote

Old   February 15, 2017, 13:59
Default
  #34
New Member
 
bangun
Join Date: Feb 2015
Posts: 16
Rep Power: 8
eb19 is on a distinguished road
Quote:
Originally Posted by anishtain4 View Post
Hi,

Since there is no clear example of dynamic Lagrangian LES model in the OpenFOAM tutorials, I attached a case I had to make work.
This is for OpenFOAM 3.0.1,
Let me know if you have any questions about it.

The codes to run it are as follow:

Code:
cp -r 0.org 0;
blockMesh;
perturbUChannel;
pimpleFoam;
One also needs
Hi Mahdi,

In the 0 folder of your test case, you included nut and nuTilda. I tried my model following your test case, and it gave error because nuSgs file is missing in the 0 folder. ( I use OpenFoam v2.3). I tried replacing nut and nuTilda with nuSgs. The simulation well. Which one is actually necessary to include? I guess this model dynamically quantifies the nuSgs (eddy viscosity based on smagorinsky coefficient). Can you please kindly explain this part? Thanks
eb19 is offline   Reply With Quote

Old   February 15, 2017, 17:17
Default
  #35
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Location: NB, Canada
Posts: 272
Rep Power: 15
anishtain4 is on a distinguished road
Quote:
Originally Posted by Adlak View Post
While running dynamicLagrangian model i am getting following error :

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[flm[0 4 -5 0 0 0 0] ] + [flm[1 1 -5 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /mnt/home/SW/CFDSupportFOAM3.0/OpenFOAM-3.0.x/src/finiteVolume/lnInclude/fvMatrix.C at line 1295.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) at ??:?
#3 Foam::tmp<Foam::fvMatrix<double> > Foam:perator+<double>(Foam::tmp<Foam::fvMatrix<d ouble> > const&, Foam::tmp<Foam::fvMatrix<double> > const&) at ??:?
#4 Foam::LESModels::dynamicLagrangian<Foam::EddyDiffu sivity<Foam::ThermalDiffusivity<Foam::Compressible TurbulenceModel<Foam::fluidThermo> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?
Aborted (core dumped)

Can anyone help me ?
This says the dimension in the flm is set wrong, I tried the case I've attached here again in OF 3.0+ and 1606, works on both fine. Not sure what's your problem.
anishtain4 is offline   Reply With Quote

Old   April 24, 2017, 16:35
Default compressible dynamicLagrangian SGS
  #36
New Member
 
Zaffar Maradona
Join Date: Nov 2014
Posts: 5
Rep Power: 9
Zaffar is on a distinguished road
Hi, I am trying to use compressible dynamicLagrangian SGS model.

Apparently, “dynamicLagrangian” has been implemented in OpenFOAM version 4.0 for both compressible and incompressible flows.

I wonder how the fmm and flm should look like in zero directory and also what are the dimensions of those two quantiles for compressible solver.

In addition, have you had any successful experience with compressible “dynamicLagrangian” SGS model?

Thanks a lot for all the help and guidance.
Zaffar is offline   Reply With Quote

Old   April 25, 2017, 02:22
Default
  #37
Member
 
Mukesh Adlak
Join Date: Jun 2016
Posts: 32
Rep Power: 7
Adlak is on a distinguished road
Quote:
Originally Posted by Zaffar View Post
Hi, I am trying to use compressible dynamicLagrangian SGS model.

Apparently, “dynamicLagrangian” has been implemented in OpenFOAM version 4.0 for both compressible and incompressible flows.

I wonder how the fmm and flm should look like in zero directory and also what are the dimensions of those two quantiles for compressible solver.

In addition, have you had any successful experience with compressible “dynamicLagrangian” SGS model?

Thanks a lot for all the help and guidance.

Hi Zaffar,
I have succesfully tested dynamicLagrangian model in OpenFOAM-3.0.x after little modification which was required for compressible flows. It was running well for incompressible flows but not for compressible flows. So I modified fmm and flm equations (Just put the density inside derivatives). I am attaching flm and fmm files for zero folder please check it, it might be helpful for u.
Attached Files
File Type: gz files.tar.gz (586 Bytes, 59 views)
Adlak is offline   Reply With Quote

Old   April 25, 2017, 19:03
Default
  #38
New Member
 
Zaffar Maradona
Join Date: Nov 2014
Posts: 5
Rep Power: 9
Zaffar is on a distinguished road
Thank you for your reply Adlak,

From OF4.0 source, you can see that "rho" variable already implemented in both equations for fmm and flm as:

Code:
    volScalarField invT
    (
        alpha*rho*(1.0/(theta_.value()*this->delta()))*pow(flm_*fmm_, 1.0/8.0)
    );

    volScalarField LM(L && M);

    fvScalarMatrix flmEqn
    (
        fvm::ddt(alpha, rho, flm_)
      + fvm::div(alphaRhoPhi, flm_)
     ==
        invT*LM
      - fvm::Sp(invT, flm_)
      + fvOptions(alpha, rho, flm_)
    );

    flmEqn.relax();
    fvOptions.constrain(flmEqn);
    flmEqn.solve();
    fvOptions.correct(flm_);
    bound(flm_, flm0_);

    volScalarField MM(M && M);

    fvScalarMatrix fmmEqn
    (
        fvm::ddt(alpha, rho, fmm_)
      + fvm::div(alphaRhoPhi, fmm_)
     ==
        invT*MM
      - fvm::Sp(invT, fmm_)
      + fvOptions(alpha, rho, fmm_)
    );

    fmmEqn.relax();
    fvOptions.constrain(fmmEqn);
    fmmEqn.solve();
    fvOptions.correct(fmm_);
    bound(fmm_, fmm0_);

    correctNut(gradU);
}
I tried fmm and flm dimensions similar to your files too but the dimensional error persists. I tested many different cases but it seems that there is a problem with dynamicLagrangian for compressible solver in OpenFOAM-4.0.

Any comments or suggestions would be greatly appreciated
Zaffar is offline   Reply With Quote

Old   April 27, 2017, 03:00
Default
  #39
Member
 
Mukesh Adlak
Join Date: Jun 2016
Posts: 32
Rep Power: 7
Adlak is on a distinguished road
Quote:
Originally Posted by Zaffar View Post
Thank you for your reply Adlak,

From OF4.0 source, you can see that "rho" variable already implemented in both equations for fmm and flm as:

Code:
    volScalarField invT
    (
        alpha*rho*(1.0/(theta_.value()*this->delta()))*pow(flm_*fmm_, 1.0/8.0)
    );

    volScalarField LM(L && M);

    fvScalarMatrix flmEqn
    (
        fvm::ddt(alpha, rho, flm_)
      + fvm::div(alphaRhoPhi, flm_)
     ==
        invT*LM
      - fvm::Sp(invT, flm_)
      + fvOptions(alpha, rho, flm_)
    );

    flmEqn.relax();
    fvOptions.constrain(flmEqn);
    flmEqn.solve();
    fvOptions.correct(flm_);
    bound(flm_, flm0_);

    volScalarField MM(M && M);

    fvScalarMatrix fmmEqn
    (
        fvm::ddt(alpha, rho, fmm_)
      + fvm::div(alphaRhoPhi, fmm_)
     ==
        invT*MM
      - fvm::Sp(invT, fmm_)
      + fvOptions(alpha, rho, fmm_)
    );

    fmmEqn.relax();
    fvOptions.constrain(fmmEqn);
    fmmEqn.solve();
    fvOptions.correct(fmm_);
    bound(fmm_, fmm0_);

    correctNut(gradU);
}
I tried fmm and flm dimensions similar to your files too but the dimensional error persists. I tested many different cases but it seems that there is a problem with dynamicLagrangian for compressible solver in OpenFOAM-4.0.

Any comments or suggestions would be greatly appreciated



Hi,
I have already installed and checked OF4.0 and OF4.x both but I haven't seen any changes. Please check this file in the installed version on ur system. Also send me the complete folder of dynamicLagrangian turbulence model at adlak@iitk.ac.in
Adlak is offline   Reply With Quote

Old   September 23, 2017, 04:41
Default
  #40
Member
 
Robert Ong
Join Date: Aug 2010
Posts: 86
Rep Power: 13
rob3rt 0ng is on a distinguished road
Quote:
Originally Posted by Zaffar View Post
Thank you for your reply Adlak,

From OF4.0 source, you can see that "rho" variable already implemented in both equations for fmm and flm as:

Code:
    volScalarField invT
    (
        alpha*rho*(1.0/(theta_.value()*this->delta()))*pow(flm_*fmm_, 1.0/8.0)
    );

    volScalarField LM(L && M);

    fvScalarMatrix flmEqn
    (
        fvm::ddt(alpha, rho, flm_)
      + fvm::div(alphaRhoPhi, flm_)
     ==
        invT*LM
      - fvm::Sp(invT, flm_)
      + fvOptions(alpha, rho, flm_)
    );

    flmEqn.relax();
    fvOptions.constrain(flmEqn);
    flmEqn.solve();
    fvOptions.correct(flm_);
    bound(flm_, flm0_);

    volScalarField MM(M && M);

    fvScalarMatrix fmmEqn
    (
        fvm::ddt(alpha, rho, fmm_)
      + fvm::div(alphaRhoPhi, fmm_)
     ==
        invT*MM
      - fvm::Sp(invT, fmm_)
      + fvOptions(alpha, rho, fmm_)
    );

    fmmEqn.relax();
    fvOptions.constrain(fmmEqn);
    fmmEqn.solve();
    fvOptions.correct(fmm_);
    bound(fmm_, fmm0_);

    correctNut(gradU);
}
I tried fmm and flm dimensions similar to your files too but the dimensional error persists. I tested many different cases but it seems that there is a problem with dynamicLagrangian for compressible solver in OpenFOAM-4.0.

Any comments or suggestions would be greatly appreciated
Hi Zaffar,
I'm getting the same incompatible dimension error.
Have you managed to solve it?
Thanks
Robert
rob3rt 0ng is offline   Reply With Quote

Reply

Tags
dynlagrangian, les, sgs

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
multiphaseInterFoam for RAS turbulence model chiven OpenFOAM Bugs 8 December 6, 2017 03:08
Wrong calculation of nut in the kOmegaSST turbulence model FelixL OpenFOAM Bugs 27 March 27, 2012 10:02
help for different between les model (subgrid-scale model) liuyuxuan FLUENT 1 October 2, 2009 16:25
2 stage axial turbine model convergence issues sherifkadry CFX 2 September 7, 2009 21:51
multi fluid mixture model issue rystokes CFX 3 August 9, 2009 20:13


All times are GMT -4. The time now is 07:16.