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

Nonlinear turbulence model NonlinearShih

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 21, 2010, 06:32
Default Nonlinear turbulence model NonlinearShih
  #1
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi all,

I've simulated a fully developed channel flow with the nonlinear shih model. The residuals are quite good (R<10e-7). But looking at the pressure it isn't constant over the channel-hight and looking at the veloicty in y-direction, they are nonzero. I have simulated this channel flow with a low-Reynolds-turbulence model and showed the different results in the following plot.

I have seen results that look nearly the same with the LRR model... Maybe it's because of the pressure near the walls. For BC I'm using zeroGradient for walls and the outlet, for inlet a fixed Value.
I'm using OpenFOAM 1.6 with directMapped bc's for U,k,epsilon at the inlet. The solver is simpleFoam. If someone has any hind please let me know.

Best regards,

Thomas
Thomas Baumann is offline   Reply With Quote

Old   July 15, 2010, 03:13
Default
  #2
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi all,

I have simulated a fully developed channel flow using the solver boundaryFoam. Here I have no problems and I get good results using for turbulence modelling NonlinearKEShih or the LienCubicKELowRe.

But starting a simulation with simpleFoam or pisoFoam I get bad results as described above.

Has anybody solved any flow with walls without this problem using simpleFoam or any solver regarding convection?

Thanks a lot,
Thomas
Thomas Baumann is offline   Reply With Quote

Old   July 23, 2010, 10:52
Default
  #3
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi all,

I'm nut sure, but could it be the problem of the simple or the piso-algorithm?

I have seen in buoyantboussinesqSimpleFoam that if an additional term is added in the U-equation (here the buoancy-term), that
this term has to be added as flux in phi, too.

In the Navier-Stokes-equations I get here the additional buoancy-term:
g*rho_delta in the U-equation.

And the flux phi is corrected with this term, which is needed for the p-equation:
surfaceScalarField ghf("ghf", g & mesh.Cf());
surfaceScalarField buoyancyPhi = rUAf *ghf*fvc::snGrad(rhok)*mesh.magSf();

phi = phi - buoyancyPhi;

...

Normal turbulence models like the k-epsilon are modelling the turbulence isotropic and because of that, the Reynolds-stresses have not to be regarded in the poisson-equation of the pressure, the same as the viscous stresses. You get the poisson-equation by
div(Navier-Stokes-equations). But in nonlinear turbulence-models and algebraic stress models they are nonzero.
So I have to split my turbulence in a isotropic and the nonisotropic part. And I have to calculate a phi_nonisotropic and have to add it to the phi. I'm not sure if that's right.
Can anybody help me?

Thank you very much,

Thomas



Regards Thomas
Thomas Baumann is offline   Reply With Quote

Old   August 5, 2010, 05:17
Default
  #4
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi all,

I have modified the mySimpleFoam-solver to calculate the residuals of continuity-equation about div(U) and the orginal one div(phi), too.

The residuals of div(phi) are about 10^-09,
but the residuals of div(U) are about 0.7

If I'm simulating using an isotropic turbulence-model for example the LaunderSharma I get
div(phi) are about 10^-09,
the residuals of div(U) are about 10^-04. So they are much better here.

The problem of the simple and the piso-algorithmus is, that they are calculating the the pressure-equation using phi.

fvScalarMatrix pEqn
(
fvm::laplacian(1.0/AU, p) == fvc::div(phi)
);

and correct the fluxes afterwards
if (nonOrth == nNonOrthCorr)
{
phi -= pEqn.flux();
}


I have seen in the posting
pimpleFoam Body Force
that you can built an additional force to the NS and pressure-equation.
So could it be possible to solve the divdevReff of the turbulence-model isotropic and add the additional explicit nonlinear-part like a force?

Regards Thomas
Thomas Baumann is offline   Reply With Quote

Old   August 30, 2010, 09:48
Default
  #5
New Member
 
Olli
Join Date: Mar 2010
Location: Berlin
Posts: 12
Rep Power: 7
Moelfus is on a distinguished road
Hi Thomas,

maybe there is something wrong with your BC's. I used the anisotropic model and it works perfectly for my needs. I used the following BC's:

U:

INLET
{
type fixedValue;
value uniform (.619552 0 0);
}

WALL
{
type fixedValue;
value uniform (0 0 0);
}

OUTLET
{
type zeroGradient;
}


p:

INLET
{
type zeroGradient;
}
WALL
{
type zeroGradient;
}
OUTLET
{
type fixedValue;
value uniform 0;
}

epsilon:

INLET
{
type fixedValue;
value uniform .0003532;
}

WALL
{
type zeroGradient;
}
OUTLET
{
type zeroGradient;
}

k:

INLET
{
type fixedValue;
value uniform .000605;
}

WALL
{
type zeroGradient;
}
OUTLET
{
type zeroGradient;
}

nut:

INLET
{
type calculated;
value uniform 0;
}

WALL
{
type nutWallFunction;
value uniform 0;
}
OUTLET
{
type calculated;
value uniform 0;
}

nuTilda:
INLET
{
type fixedValue;
value uniform 0;
}
WALL
{
type zeroGradient;
}
OUTLET
{
type zeroGradient;
}

Is your mesh 2d or 3d? Are the dimensions/scaling of the domain right? Are the results mesh independent? What is the Reynoldsnumber? ... This would be some questions I'd usually ask.

Best regards,

Olli
Moelfus 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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
SimpleFoam case with SpalartAllmaras turbulence model implemented nedved OpenFOAM Running, Solving & CFD 2 November 30, 2014 23:43
Adding a Turbulence Model doug OpenFOAM Running, Solving & CFD 10 October 2, 2012 06:55
KOmega Turbulence model from wwwopenFOAMWikinet philippose OpenFOAM Running, Solving & CFD 30 August 4, 2010 10:26
v2-f turbulence model in CFX? flga CFX 14 November 23, 2006 07:12


All times are GMT -4. The time now is 00:39.