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

Initialize the field using another simpler turbolence model

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 13, 2014, 21:58
Default Initialize the field using another simpler turbolence model
  #1
Member
 
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5
ArathoN is on a distinguished road
hi foamers,

My friend told me that in Fluent there is an option to initialize the flow properties then run the desired the simulation. I searched for such an option on openfoam but i found nothing.

So i was thinking if i use a 1ep.-model like spalart-allmaras to initialize the flow then i swith to my desired RAS model, Does this improve my solution? and more importantly does the solution converge faster?
ArathoN is offline   Reply With Quote

Old   February 20, 2014, 14:51
Default
  #2
Member
 
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5
ArathoN is on a distinguished road
Resolved.

First before running any simulation use:
Code:
refineMesh
It will help the first steps of the simulation.

Then if you use kEpsilon, it's better to run potentialFoam to initialize the U & p fields, you need to add this in the fvsolution file
Code:
potentialFlow
{
    nNonOrthogonalCorrectors 10;
}
then run
Code:
potentialFoam
Finally if you'll use the kOmegaSST initialize the fields with the data from the kEpsilon, the same with every other model derived from the kEpsilon. In genereal the kEpsilon is the fastest one so it's better to use it then feed the data to the others and the gain in cpu time reduction is huge.

That's all i learned. If some one has more advice i'll gladly hear him.

Last edited by ArathoN; February 21, 2014 at 10:08. Reason: fix a typo
ArathoN is offline   Reply With Quote

Old   February 21, 2014, 05:47
Default
  #3
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 891
Rep Power: 14
RodriguezFatz will become famous soon enough
Quote:
Originally Posted by ArathoN View Post
Then if you use kEpsilon, it's better to run potentialFoam to initialize the U & p fields, you need to add this in the fvsolution file
Code:
potentialFlow
{
    nNonOrthogonalCorrectors 10;
}
Hi, i think this is exactly what Fluent does when using "Hybrid Initialization".
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   February 21, 2014, 10:07
Default
  #4
Member
 
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5
ArathoN is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
Hi, i think this is exactly what Fluent does when using "Hybrid Initialization".
Exactly I have a friend using fluent and old me about this initialization so after some test and research i found out how to do it in openFoam. In the case of kEpsilon running potentialFoam before the main solver has little effect (at least for the cases i studied), but in case of different models (LaunderSharmaLowRe, kOmegaSST,....) the initialization with kEpsilon helps really in reducing the time needed for the convergence.
ArathoN is offline   Reply With Quote

Old   February 24, 2014, 02:41
Default
  #5
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 891
Rep Power: 14
RodriguezFatz will become famous soon enough
Aditionally to the speedup, I also had a case that diverged with a simple constant initialization but not with the potentialFoam init.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   February 27, 2014, 10:22
Default
  #6
Member
 
ArathoN
Join Date: Jul 2011
Posts: 86
Rep Power: 5
ArathoN is on a distinguished road
Quote:
Originally Posted by RodriguezFatz View Post
Aditionally to the speedup, I also had a case that diverged with a simple constant initialization but not with the potentialFoam init.
If you use very accurate schemes, sometimes the case will diverge. It's better to start the simulation with a diffusive scheme but robust, then after some iterations switch to the accurate one. That's what i do when i need to simulate complex cases.
ArathoN is offline   Reply With Quote

Old   March 2, 2014, 21:55
Default
  #7
Member
 
Baris (Heewa)
Join Date: Jan 2013
Location: Japan
Posts: 86
Rep Power: 3
shipman is on a distinguished road
Dear Arathon,

I also try to initialize my flow field using potentialflow before running my multiphase calculation according to your above explanation, but i couldnt succeed. in multiphase pressure dimension is kgm/s^2 however in potetialflow it is m^2/s^2. i set my cases as follows and but giving following error (is it error or not no idea). also how can i initialize the value of k and epsilon?? could you help to me pls...thanks

==>0/U
Code:
dimensions      [0 1 -1 0 0];
internalField   uniform (0 0 0);
boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform (0 -3.104 0);
    }
    outlet
    {
        type            zeroGradient;
    }
    wall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
=>0/P
dimensions [0 2 -2 0 0 0 0];
Code:
internalField   uniform 0;
boundaryField
{
    inlet
    {
         type           zeroGradient;
    }
    outlet
    {
        type            fixedValue;
        value           $internalField;;
    }
    wall
    {
         type            zeroGradient;
    }
==> fvSchemes:
Code:
ddtSchemes
{
    default              steadyState;
}

interpolationSchemes
{
   default         linear;
    interpolate(U)  linear;
}

divSchemes
{
    default              none;
   div(phi,U)      Gauss upwind;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div(phi,nuTilda) Gauss upwind;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}
gradSchemes
{
    default              Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
    laplacian(nuEff,U) Gauss linear corrected;
     laplacian(1,p)  Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

snGradSchemes
{
 default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}
==>fvsolution:
Code:
solvers
{
   "(U|k|omega)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-06;
        relTol          0;
    }
   p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0;
    }
}

potentialFlow
{
nNonOrthogonalCorrectors   10;
}
sorry i forgat to paste the error:

DICPCG: Solving for p, Initial residual = 1, Final residual = 8.80882e-07, No Iterations 180
DICPCG: Solving for p, Initial residual = 0.168621, Final residual = 9.37342e-07, No Iterations 131
DICPCG: Solving for p, Initial residual = 0.00789625, Final residual = 9.67837e-07, No Iterations 115
DICPCG: Solving for p, Initial residual = 0.000384399, Final residual = 8.94174e-07, No Iterations 101
DICPCG: Solving for p, Initial residual = 2.60676e-05, Final residual = 8.91063e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 1.92316e-06, Final residual = 5.88908e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 7.12976e-07, Final residual = 7.12976e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 7.12976e-07, Final residual = 7.12976e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 7.12976e-07, Final residual = 7.12976e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 7.12976e-07, Final residual = 7.12976e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 7.12976e-07, Final residual = 7.12976e-07, No Iterations 0
continuity error = 0.0244929
Interpolated U error = 0.000203337
ExecutionTime = 6.04 s ClockTime = 6 s
shipman 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
How to implement compressibility correction factor in k-epsilon model neeraj OpenFOAM Programming & Development 3 October 15, 2012 00:53
how to model a movable droplet sourse in electirc field Chande FLOW-3D 1 March 12, 2011 17:49
DPM model w/ Wave model - errors in documentation HS FLUENT 0 April 12, 2006 04:37
just a question about airfoil (Turbolence model and Cd) Maria Teresa Milesi FLUENT 3 April 7, 2000 09:56
I wish to find the proper model to validate the temperature field. G.H.Lee Main CFD Forum 1 May 6, 1999 02:05


All times are GMT -4. The time now is 22:03.