Description: Although LRR is
 

Description:
Although LRR is a valid choice in const/turbulenceProperties, the case doesn't run.

Solver/Application:
rasInterFoam

Source file:

(if possible name of OpenFOAM library and file in the library)

Testcase:
Case : damBreak

Platform:
SLED 10 (SuSE)
amd64

Version:
1.4.1

Notes:
Nprocs : 1
Create time

Create mesh for time = 0


Reading environmentalProperties
Reading field pd

Reading field gamma

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Calculating field g.h

Selecting turbulence model LRR


--> FOAM FATAL IO ERROR : unexpected class name volTensorField expected volSymmTensorField
while reading object R

file: /tirian10/lokal/OpenFOAM/dragosm-1.4.1/run/tutorials/rasInterFoam//damBreak/0/R at line 21.

From function regIOobject::readStream(const word&)
in file db/regIOobject/regIOobjectRead.C at line 113.

FOAM exiting

I tried kEpsilon, RNGkEpsilon, NonlinearKEShih models, and they run well.

Try replacing volTensorField w
 

Try replacing volTensorField with volSymmTensorField in the file /tirian10/lokal/OpenFOAM/dragosm-1.4.1/run/tutorials/rasInterFoam//damBreak/0/R

I will fix the file for the next release.

Ok, it was that simple...http:
 

Ok, it was that simple...http://www.cfd-online.com/OpenFOAM_D...part/happy.gif, and it wasn't actually a bug.
Well, for the information to be completed, it is necessary to change the specification of the tensor, too. In the same file the following occurences (0 0 0 0 0 0 0 0 0) have to be replaced with (0 0 0 0 0 0). Since it is a symmetric tensor, it needs only 6 value to be completely defined.

And by the way, thank you Henry!

...but the problems are still
 

...but the problems are still there http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif.
If I keep the default settings (which work for the 2 equation models) I still get a solution, but not a physical one.
http://www.cfd-online.com/OpenFOAM_D...s/126/6008.jpg

Lowering the MaxCo from 0.2 to 0.02 or even lower, makes the things even worse: the computation ends with a floating point exception. Switching the discretization schemes from Gauss linear to Gauss upwind doesn't help, the same floating point exception occurs at the end.
Anybody could give me a hint on how to tackle this thing?

Dragos

Hey.. Am having a problem with simulating using LRR turbulence model in transientSimpleFoam!!
The timeStepContinuityError blows out of proportion and the simulation stops! Kindly tell me if you have any solution to this problem!!

Hi users, I am using OF 1.4.1 rasInterFoam solver with LRR turbulence model on damBreak case. I replaced volTensorField with volSymmTensorField in the R file but simulation stops and floating exception occurs.

Could be due to a bug in LRR.C file? There are some commented lines in Dissipation and Reynolds stress equations in LRR.C. Do they have to be commented?

// Dissipation equation
tmp<fvScalarMatrix> epsEqn
(
fvm::ddt(epsilon_)
+ fvm::div(phi_, epsilon_)
//- fvm::laplacian(Ceps*(K/epsilon_)*R, epsilon_)
- fvm::laplacian(DepsilonEff(), epsilon_)
==
C1*G*epsilon_/k_
- fvm::Sp(C2*epsilon_/k_, epsilon_)
);

epsEqn().relax();

....

// Reynolds stress equation

const fvPatchList& patches = mesh_.boundary();

forAll(patches, patchi)
{
const fvPatch& curPatch = patches[patchi];

if (typeid(curPatch) == typeid(wallFvPatch))
{
forAll(curPatch, facei)
{
label faceCelli = curPatch.faceCells()[facei];
P[faceCelli]
*= min(G[faceCelli]/(0.5*tr(P[faceCelli]) + SMALL), 1.0);
}
}
}


tmp<fvSymmTensorMatrix> REqn
(
fvm::ddt(R_)
+ fvm::div(phi_, R_)
//- fvm::laplacian(Cs*(k_/epsilon_)*R_, R_)
- fvm::laplacian(DREff(), R_)
+ fvm::Sp(Clrr1*epsilon_/k_, R_)
==
P
- (2.0/3.0*(1 - Clrr1)*I)*epsilon_
- Clrr2*dev(P)
);

REqn().relax();


Thanks in advance
Martín.

Try it with OpenFOAM-1.6.x.

H

R field in dambrak tutorial openfoam
 

Hi,

I'm was looking on the ras dambreak tutorial. In the /0 dir, there are a lot of boundary conditions set. Alpha1, k, epsilon, U and p_rgh are logical. But what are nut (normaly calculated from k and epsilon), mut, nuTilda and R doing there? What is the physical meaning of R [m2/s2] and mud [kg/m/s]? Is there amy documentation where I can find what is solved there?

Thx!!