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

Convergence problem with tetrahedral grids

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

Like Tree1Likes
  • 1 Post By hjasak

Reply
 
LinkBack Thread Tools Display Modes
Old   December 2, 2010, 18:58
Default Convergence problem with tetrahedral grids
  #1
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 6
Tarak is on a distinguished road
Hii,

I am running the case of flow over a square cylinder using LES by ICEM generated grid. But only after a few time steps, the code diverges, with Courant number crossing 4 or 5. I tried to use Upwind Schemes as well as first order time stepping to tackle the problem, but still the issue wasn't solved. At last, I increased the number of PISO non-orthogonal correctors to 5 (since increasing to 3 didn't help), and now its converging, but its painstakingly slow.

Can you please let me know of a way by which I can run OF with tethrahedral grids smoothly.

Thanks,
Tarak
Tarak is offline   Reply With Quote

Old   December 3, 2010, 05:28
Default
  #2
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
I am also facing difficulties on getting a 3D tetra mesh converging with OF 1.6.x.
The case is quite standard: some pipes with two fans that put the fluid in motion. The geometry is complex and I have no possibility to use a hexa mesh. The case is steady state and turbulent (simpleFoam); BC are as tested on similar (working) cases.
fvSchemes are:
Code:
gradSchemes: faceMDLimited Gauss linear 0.5;
divSchemes: Gauss linearUpwind cellLimited Gauss linear 1;
laplacianSchemes: Gauss linear limited 0.5;
fvSolution:
Code:
p
    {
        solver          GAMG;
        tolerance       1e-12;
        relTol          0;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U - epsilon - k
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-10;
        relTol          0;
    }

SIMPLE
{
    nNonOrthogonalCorrectors 2;
    pRefCell        0;
    pRefValue       0;
}

relaxationFactors  ///really low in the beginning to let the simulation start.
{
    default         0;
    p               0.05;
    U               0.2;
    k               0.2;
    epsilon            0.2;
    nuTilda            0.3;
}
The solution converges for the first 150 steps nicely, but after on it start to get unstable and finally crashes. I really do not know what to do for keep it running...
Suggestions?

mad
maddalena is offline   Reply With Quote

Old   December 3, 2010, 05:54
Default
  #3
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by maddalena View Post
I am also facing difficulties on getting a 3D tetra mesh converging with OF 1.6.x.
The case is quite standard: some pipes with two fans that put the fluid in motion. The geometry is complex and I have no possibility to use a hexa mesh. The case is steady state and turbulent (simpleFoam); BC are as tested on similar (working) cases.
fvSchemes are:
Code:
gradSchemes: faceMDLimited Gauss linear 0.5;
divSchemes: Gauss linearUpwind cellLimited Gauss linear 1;
laplacianSchemes: Gauss linear limited 0.5;
fvSolution:
Code:
p
    {
        solver          GAMG;
        tolerance       1e-12;
        relTol          0;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U - epsilon - k
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-10;
        relTol          0;
    }

SIMPLE
{
    nNonOrthogonalCorrectors 2;
    pRefCell        0;
    pRefValue       0;
}

relaxationFactors  ///really low in the beginning to let the simulation start.
{
    default         0;
    p               0.05;
    U               0.2;
    k               0.2;
    epsilon            0.2;
    nuTilda            0.3;
}
The solution converges for the first 150 steps nicely, but after on it start to get unstable and finally crashes. I really do not know what to do for keep it running...
Suggestions?

mad
Hi Maddalena,
if you are using linearUpwind for all the divSchemes, try instead to set div(phi,U) to Gauss linearUpwindV faceMDLimited Gauss linear 1, and div(phi,k/epsilon) to Gauss upwind. By the way, why so strong underrelaxation factors? Have you tried to leave the URF for p at the 0.3 standard value, for U at 0.7 and to set the URF's for k and epsilon to 0.4-0.5?

Best Regards

Vesselin
vkrastev is offline   Reply With Quote

Old   December 3, 2010, 05:57
Default
  #4
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by Tarak View Post
Hii,

I am running the case of flow over a square cylinder using LES by ICEM generated grid. But only after a few time steps, the code diverges, with Courant number crossing 4 or 5. I tried to use Upwind Schemes as well as first order time stepping to tackle the problem, but still the issue wasn't solved. At last, I increased the number of PISO non-orthogonal correctors to 5 (since increasing to 3 didn't help), and now its converging, but its painstakingly slow.

Can you please let me know of a way by which I can run OF with tethrahedral grids smoothly.

Thanks,
Tarak
Hi Tarak,
two hints: 1) use hexa-meshes for LES calculations; 2) you cannot use first order schemes for LES, because they are too diffusive: you'll have to use at least a limited second order scheme, such as limitedLinear.

Best regards

Vesselin
vkrastev is offline   Reply With Quote

Old   December 3, 2010, 06:02
Default
  #5
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by vkrastev View Post
By the way, why so strong underrelaxation factors? Have you tried to leave the URF for p at the 0.3 standard value, for U at 0.7 and to set the URF's for k and epsilon to 0.4-0.5?
Oops, I haven't noticed the comment in the fvSolution dictionary So
, let me change the question: what are your URF's after the first n-steps in which you leave so low values?
vkrastev is offline   Reply With Quote

Old   December 3, 2010, 06:29
Default
  #6
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by vkrastev View Post
what are your URF's after the first n-steps in which you leave so low values?
Unfortunately, I cannot get too far to have the time to increase them! After 120 steps the solution starts to be unstable, thus increase them sounds as not a good idea...
Quote:
Originally Posted by vkrastev View Post
div(phi,k/epsilon) to Gauss upwind
you want to increase diffusion of turbulence quantities, do not you?

BTW... sounds a bit weird that, whenever I change my fvSchemes & fvSolution, I cannot get too far with my simulation. May there be something more subtle than this? May be due to the 2 fan BC I imposed?


mad

PS: seems like in the last day we are the only active people in the forum
maddalena is offline   Reply With Quote

Old   December 3, 2010, 07:37
Default
  #7
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by maddalena View Post
you want to increase diffusion of turbulence quantities, do not you?
Yes, It's a matter of trade-off between accuracy and stability: I've noticed in some of my runs that changing only the div(phi,U) scheme to something more accurate than the first order upwind, gives very significant improvements to the results comparing with an all-upwind setting for the divSchemes. On the other hand, till now, with tetra-dominant meshes I was not able to reach satisfactory convergemce patterns for k and epsilon with higher order schemes...So, better a quite accurate and converging result, than a very accurate but no-converging-at-all result...

Quote:
Originally Posted by maddalena View Post
BTW... sounds a bit weird that, whenever I change my fvSchemes & fvSolution, I cannot get too far with my simulation. May there be something more subtle than this? May be due to the 2 fan BC I imposed?
Yes, the problem could be easily far from the fvSchemes/Solution tuning (what is your checkMesh "opinion" about it?)...unfortunately I have no experience with fan BC's, so I cannot give you any useful advice...


Quote:
Originally Posted by maddalena View Post
PS: seems like in the last day we are the only active people in the forum
So it seems...

Vesselin
vkrastev is offline   Reply With Quote

Old   December 3, 2010, 08:33
Default
  #8
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by vkrastev View Post
better a quite accurate and converging result, than a very accurate but no-converging-at-all result...
Especially if you have some close-by deadlines...
Quote:
Originally Posted by vkrastev View Post
what is your checkMesh "opinion" about it?
Code:
    Overall domain bounding box (-12 -1.804 -7.19731e-17) (14.905 1.804 10.0839)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-3.66027e-18 -7.23166e-17 -1.6178e-15) OK.
    Max cell openness = 2.94713e-16 OK.
    Max aspect ratio = 7.21422 OK.
    Minumum face area = 2.38932e-06. Maximum face area = 0.734457.  Face area magnitudes OK.
    Min volume = 2.87124e-09. Max volume = 0.183334.  Total volume = 327.312.  Cell volumes OK.
    Mesh non-orthogonality Max: 65.408 average: 20.4121
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.763815 OK.
checkMesh says that the problem lies somewhere else...
I will give a try to upwind on k and epsilon. Thank you in the meanwhile..

mad
maddalena is offline   Reply With Quote

Old   December 3, 2010, 09:25
Default
  #9
Senior Member
 
Vesselin Krastev
Join Date: Jan 2010
Location: University of Tor Vergata, Rome
Posts: 361
Rep Power: 10
vkrastev is on a distinguished road
Quote:
Originally Posted by maddalena View Post
Especially if you have some close-by deadlines...
That's for sure!

Quote:
Originally Posted by maddalena View Post
Code:
    Overall domain bounding box (-12 -1.804 -7.19731e-17) (14.905 1.804 10.0839)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-3.66027e-18 -7.23166e-17 -1.6178e-15) OK.
    Max cell openness = 2.94713e-16 OK.
    Max aspect ratio = 7.21422 OK.
    Minumum face area = 2.38932e-06. Maximum face area = 0.734457.  Face area magnitudes OK.
    Min volume = 2.87124e-09. Max volume = 0.183334.  Total volume = 327.312.  Cell volumes OK.
    Mesh non-orthogonality Max: 65.408 average: 20.4121
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.763815 OK.
checkMesh says that the problem lies somewhere else...
I agree with "him"

Quote:
Originally Posted by maddalena View Post
I will give a try to upwind on k and epsilon. Thank you in the meanwhile..
Good luck!

V
vkrastev is offline   Reply With Quote

Old   December 6, 2010, 13:33
Default
  #10
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 418
Rep Power: 14
santiagomarquezd will become famous soon enough
Hi Tarak, Did you try renumberMesh after importing the mesh to FOAM? I've found that meshes imported from Fluent are not very efficient in the numeration and this impacts strongly in iterative solvers.

Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Post-doctoral Fellow
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
http://www.cimec.org.ar

Last edited by santiagomarquezd; December 6, 2010 at 13:35. Reason: Spelling
santiagomarquezd is offline   Reply With Quote

Old   December 7, 2010, 03:09
Default
  #11
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by santiagomarquezd View Post
Hi Tarak, Did you try renumberMesh after importing the mesh to FOAM? I've found that meshes imported from Fluent are not very efficient in the numeration and this impacts strongly in iterative solvers.
NB: this will not work if you have cyclic patch! When renumbering mesh, the cyclics will be lost!

mad
maddalena is offline   Reply With Quote

Old   February 7, 2011, 04:38
Default suggestions?
  #12
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hi everybody,
seems like all my problems are still there, on a case that is similar to what posted above. I wrote on a different thread: pressure eq. "converges" after few time steps
Maybe you can take a look to it and suggest something more on the subject...

mad
maddalena is offline   Reply With Quote

Old   February 7, 2011, 11:16
Default
  #13
Senior Member
 
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 122
Rep Power: 6
tcarrigan is on a distinguished road
This is the thread I meant to post on. I started clicking your links and posted to the wrong one . I'll repeat my post:

----------------------------------------------------------------
Just curious, have you tried using leastSquares for the gradScheme?

I did some 2D calculations for a NACA airfoil using both structured and unstructured grids. I too suffered convergence issues when running the calculation for the unstructured case. However, switching the gradScheme to a cellLimited leastSquares happened to solve the problem.

Let me know if this works.
----------------------------------------------------------------

And to answer your question, there may not be an advantage to using leastSquares, it's just an observation made from several simulations I've run for unstructured grids. Most of the time I have issues obtaining convergence when using tet grids and the Gauss linear gradScheme. Just and observation, was curious to see if it had any effect on your calculation.
tcarrigan is offline   Reply With Quote

Old   February 7, 2011, 11:20
Default
  #14
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by tcarrigan View Post
And to answer your question, there may not be an advantage to using leastSquares, it's just an observation made from several simulations I've run for unstructured grids. Most of the time I have issues obtaining convergence when using tet grids and the Gauss linear gradScheme. Just and observation, was curious to see if it had any effect on your calculation.
Ok, I'll give it a try...

mad
maddalena is offline   Reply With Quote

Old   February 7, 2011, 12:26
Default
  #15
Senior Member
 
Tarak
Join Date: Aug 2010
Location: State College, PA
Posts: 105
Rep Power: 6
Tarak is on a distinguished road
Hii,

I would recommend using Gamma Differencing Scheme with appropriate blending factor for obtaining good convergence/stability for tetrahedral grids. This is how I managed to get the code run.

Thanks,
Tarak
Tarak is offline   Reply With Quote

Old   February 9, 2011, 05:27
Default
  #16
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by tcarrigan View Post
Just curious, have you tried using leastSquares for the gradScheme?

I did some 2D calculations for a NACA airfoil using both structured and unstructured grids. I too suffered convergence issues when running the calculation for the unstructured case. However, switching the gradScheme to a cellLimited leastSquares happened to solve the problem.
So, here an answer to your observations: pressure eq. "converges" after few time steps

mad
maddalena is offline   Reply With Quote

Old   February 9, 2011, 09:57
Default
  #17
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
In 1.6-ext, we've got special discretisation scheme for tet meshes: use it on convection in the momentum equation and on interpolate(U). The scheme is called reconCentral, and the settings for a tet mesh look like this:

gradSchemes
{
default cellLimited leastSquares 1.0;
}

divSchemes
{
div(phi,U) Gauss reconCentral cellLimited leastSquares 1.0;
//...
}

laplacianSchemes
{
default Gauss linear limited 0.5;
}

interpolationSchemes
{
default linear;
interpolate(HbyA) linear;
interpolate(U) reconCentral phi cellLimited leastSquares 1.0;
}

Enjoy,

Hrv
fumiya likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak 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
convergence problem commonyue Main CFD Forum 1 December 1, 2009 04:54
Submerged fin, Convergence problem supermouniette FLUENT 10 July 6, 2009 10:47
Convergence of CFX field in FSI analysis nasdak CFX 2 June 29, 2009 01:17
convergence problem in comsol anderson Main CFD Forum 0 February 24, 2008 17:54
CONVERGENCE PROBLEM - oil boiler MM FLUENT 1 February 15, 2007 06:24


All times are GMT -4. The time now is 21:08.