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

convergence problem in using incompressible transient solvers.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 22, 2011, 01:16
Default convergence problem in using incompressible transient solvers.
  #1
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
Dear Foarmers,

Hello, I'd like to simulate the 3D half-wing which is mounted on the symmetry plane.

Recently, I applied pisoFoam and pimpleFoam to get the unsteady solutions but the solutions have been diverged.

I tried to apply those solvers with lower tolerance criteria, various solver types and schemes but they generally weren't helpful at all.

Please give me an advice on using the transient solvers.

Here I attached the control, fvSolution and fvSchemes files recently used.

controlDict :
Code:
  1 /*--------------------------------*- C++ -*----------------------------------*\
  2 | =========                 |                                                 |
  3 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
  4 |  \\    /   O peration     | Version:  1.7.1                                 |
  5 |   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
  6 |    \\/     M anipulation  |                                                 |
  7 \*---------------------------------------------------------------------------*/
  8 FoamFile
  9 {
 10     version     2.0;
 11     format      ascii;
 12     class       dictionary;
 13     location    "system";
 14     object      controlDict;
 15 }
 16 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 17 
 18 //application     simpleFoam;
 19   application     pimpleFoam;
 20 //application     pisoFoam;
 21 
 22 startFrom       latestTime;
 23 
 24 startTime       0;
 25 
 26 stopAt          endTime;
 27 
 28 endTime         200;
 29 
 30 deltaT          1e-5;
 31 
 32 writeControl    timeStep;
 33 
 34 writeInterval   100;
 35 
 36 purgeWrite      0;
 37 
 38 writeFormat     ascii;
 39 
 40 writePrecision  6;
 41 
 42 writeCompression uncompressed;
 43 
 44 timeFormat      general;
 45 
 46 timePrecision   6;
 47 
 48 runTimeModifiable yes;
 49 
 50 adjustTimeStep yes;
 51 
 52 maxCo 5;
 53 
 54 functions
 55 {
 56         forces
 57         {
 58                 type            forceCoeffs;
 59                 functionObjectLibs      ( "libforces.so" );
 60                 outputControl           timeStep;
 61                 outputInterval          1;
 62                 patches         ( wing flap );
 63                 rhoName         rhoInf;
 64                 log             true;
 65                 rhoInf          1.225;
 66                 CofR            ( 45.89 0 0 );
 67                 liftDir         ( 0 1 0 );
 68                 dragDir         ( 1 0 0 );
 69                 pitchAxis       ( 0 0 1 );      // PITCH
 70                 magUInf         2;
 71                 lRef            53.97;
 72                 Aref            3006.1;
 73         }
 74 }
 75 
 76 
 77 // ************************************************************************* //
fvSolution :
Code:
  1 /*--------------------------------*- C++ -*----------------------------------*\
  2 | =========                 |                                                 |
  3 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
  4 |  \\    /   O peration     | Version:  1.7.1                                 |
  5 |   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
  6 |    \\/     M anipulation  |                                                 |
  7 \*---------------------------------------------------------------------------*/
  8 FoamFile
  9 {
 10     version     2.0;
 11     format      ascii;
 12     class       dictionary;
 13     object      fvSolution;
 14 }
 15 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 16 
 17 solvers
 18 {
 19     p
 20     {
 21                 solver                  GAMG;
 22                 tolerance               1e-07;
 23                 relTol                  0.001;
 24                 smoother                GaussSeidel;
 25                 cacheAgglomeration      true;
 26                 nCellsInCoarsestLevel   10;
 27                 agglomerator            faceAreaPair;
 28                 mergeLevels             1;
 29     };
 30 
 31     pFinal
 32     {
 33                 solver                  GAMG;
 34                 tolerance               1e-07;
 35                 relTol                  0.001;
 36                 smoother                GaussSeidel;
 37                 cacheAgglomeration      true;
 38                 nCellsInCoarsestLevel   10;
 39                 agglomerator            faceAreaPair;
 40                 mergeLevels             1;
 41     };
 42 
 43     U
 44     {
 45                 solver                  PBiCG;
 46                 preconditioner  DILU;
 47                 tolerance               1e-08;
 48                 relTol                  0;
 49     };
 50 
 51     UFinal
 52     {
 53                 solver                  PBiCG;
 54                 preconditioner  DILU;
 55                 tolerance               1e-08;
 56                 relTol                  0;
 57     };
 58 
 59     k
 60     {
 61                 solver                  PBiCG;
 62                 preconditioner  DILU;
 63                 tolerance               1e-08;
 64                 relTol                  0;
 65     };
 66 
 67     omega
 68     {
 69                 solver                  PBiCG;
 70                 preconditioner  DILU;
 71                 tolerance               1e-08;
 72                 relTol                  0;
 73     };
 74 }
 75 
 76 SIMPLE
 77 {
 78     nNonOrthogonalCorrectors 1;
 79     pRefCell        0;
 80     pRefValue       0;
 81 }
 82 
 83 PISO
 84 {
 85         nCorrectors 5;
 86     nNonOrthogonalCorrectors 0;
 87     pRefCell        0;
 88     pRefValue       0;
 89 }
 90 
 91 PIMPLE
 92 {
 93         nOuterCorrectors 10;
 94         nCorrectors 2;
 95         nNonOrthogonalCorrectors 0;
 96     pRefCell        0;
 97     pRefValue       0;
 98 }
 99 
100 relaxationFactors
101 {
102     U           1;
103     k           1;
104     omega       1;
105 //  p  0.01;
106 //  U  0.1;
107 //  k  0.1;
108 //  omega 0.1;
109 }
110 
111 // ************************************************************************* //
fvSchemes :
Code:
  1 /*--------------------------------*- C++ -*----------------------------------*\
  2 | =========                 |                                                 |
  3 | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
  4 |  \\    /   O peration     | Version:  1.7.1                                 |
  5 |   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
  6 |    \\/     M anipulation  |                                                 |
  7 \*---------------------------------------------------------------------------*/
  8 FoamFile
  9 {
 10     version     2.0;
 11     format      ascii;
 12     class       dictionary;
 13     object      fvSchemes;
 14 }
 15 // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 16 
 17 ddtSchemes
 18 {
 19 //      default steadyState;
 20 //      default         CrankNicholson 0.5;
 21 //      default backward;
 22         default Euler;
 23 }
 24 
 25 gradSchemes
 26 {
 27     default         Gauss linear;
 28     grad(p)         Gauss linear;
 29     grad(U)         Gauss linear;
 30 //    grad(U)         cellLimited Gauss linear 1;
 31 }
 32 
 33 divSchemes
 34 {
 35     default         Gauss upwind;
 36 //  div(phi,U)      Gauss linearUpwindV Gauss linear;
 37 //  div(phi,k)      Gauss linearUpwind Gauss linear;
 38 //  div(phi,omega)  Gauss linearUpwind Gauss linear;
 39     div((nuEff*dev(grad(U).T()))) Gauss linear;
 40 }
 41 
 42 laplacianSchemes
 43 {
 44     default         Gauss linear corrected;
 45 //  default         Gauss linear limited 0.5;
 46 //  default         Gauss linear limited 0.333;
 47 }
 48 
 49 interpolationSchemes
 50 {
 51     default         linear;
 52     interpolate(U)  linear;
 53 }
 54 
 55 snGradSchemes
 56 {
 57     default         corrected;
 58 }
 59 
 60 fluxRequired
 61 {
 62     default         no;
 63     p;
 64 }
 65 
 66 // ************************************************************************* //
Regards,
Geon-Hong.

Last edited by Geon-Hong; November 22, 2011 at 05:17.
Geon-Hong is offline   Reply With Quote

Old   November 22, 2011, 04:03
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Your maximum Courant number is 5, too high. Set it to something less than 1.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 22, 2011, 05:12
Default Courant number
  #3
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
Dear alberto,

Thanks for your reply.

Of course I tried lower value of Courant number, which was set to be 0.5 or unity. However the problem was the same.

Regards,
Geon-Hong.
Geon-Hong is offline   Reply With Quote

Old   November 22, 2011, 08:41
Default One possibility
  #4
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
One possible reason is a mistake in BC's,

To investigate this, I am looking for examples and using their BC's... Or I am looking in the log file what is the diverging variable and trying to find the error there.

Another approach is to try to simplify the case. Start from a working example and add feature after feature... and when you will know the step which is causing your troubles you can deal with it.

Martin.
darai is offline   Reply With Quote

Old   November 23, 2011, 22:06
Default dear Holecek
  #5
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
Dear Holecek,

Thank you for your reply.

I tried other boundary conditions which are used in tutorial cases.

Still it doesn't work at all.

By the way, what log file should I check?

Thank you very much.

Regards,
Geon-Hong.
Geon-Hong is offline   Reply With Quote

Old   November 23, 2011, 23:17
Default
  #6
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Did you check the mesh for problems (checkMesh)?
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 24, 2011, 01:21
Default checkMesh
  #7
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
Dear Alberto,

Of course I did.

However, there is a awkward thing that,

High aspect ratio cells found

and

Failed 1 mesh checks.

But I can't find what is problem. The checkMesh result is as below,

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 1.7.1-03e7e056c215
Exec   : checkMesh
Date   : Nov 24 2011
Time   : 14:03:27
Host   : adlc11
PID    : 10513
Case   : /home/users/kgb/Work/flap/ucav1303/flap10c10b975p
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
 
Create polyMesh for time = 0
 
Time = 0
 
Mesh stats
    points:           6933336
    faces:            20575358
    internal faces:   20351362
    cells:            6821120
    boundary patches: 8
    point zones:      0
    face zones:       1
    cell zones:       1
 
Overall number of cells of each type:
    hexahedra:     6821120
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0
 
Checking topology...
    Boundary definition OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).
 
Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                  
    flap                6172     6174     ok (closed singly connected)      
    bottom              20060    20382    ok (non-closed singly connected)  
    top                 20060    20382    ok (non-closed singly connected)  
    side                29244    29508    ok (non-closed singly connected)  
    outflow             36816    37209    ok (non-closed singly connected)  
    inflow              47200    47637    ok (non-closed singly connected)  
    symPlane            28860    29223    ok (non-closed singly connected)  
    wing                35584    35685    ok (non-closed singly connected)  
 
Checking geometry...
    Overall domain bounding box (-247.502 -270 0) (900 270 358.535)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-1.03703e-16 1.14641e-15 -2.58996e-15) OK.
 ***High aspect ratio cells found, Max aspect ratio: 13183.7, number of cells 260418
  <<Writing 260418 cells with high aspect ratio to set highAspectRatioCells
    Minumum face area = 5.15158e-07. Maximum face area = 2886.02.  Face area magnitudes OK.
    Min volume = 4.04901e-08. Max volume = 71036.  Total volume = 1.94209e+08.  Cell volumes OK.
    Mesh non-orthogonality Max: 89.7243 average: 28.048
   *Number of severely non-orthogonal faces: 767159.
    Non-orthogonality check OK.
  <<Writing 767159 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 2.69123 OK.
 
Failed 1 mesh checks.
 
End
Geon-Hong is offline   Reply With Quote

Old   November 24, 2011, 01:27
Default
  #8
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
It seems you have 260418 cells with high aspect ratio, and at least one of them has an aspect ratio of 13183.7, which is extremely high.

Code:
***High aspect ratio cells found, Max aspect ratio: 13183.7, number of cells 260418   <<Writing 260418 cells with high aspect ratio to set highAspectRatioCells
The checkMesh utility should write a file listing the affected cells.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   November 24, 2011, 02:27
Default checkMesh results
  #9
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
Dear Alberto,

Yes, I checked the high aspect ratio cells from the file highAspectRatioCells in constant/polyMesh/sets.

What can I do with this cell-set? Is there any way to improve this problem?

I guess those high-aspect-ratio cells are generated from the cells adjacent to the wall.

The wing I want to simulate is tapered, which means that the wing tip has smaller chord length than the root. Furthermore, I generated the structured grid over the wing. Thus the wing has the same number of grid points along the chord at both wing tip and root. This might cause such problems, I guess.

Regeneration of the grid is only hope? ToT
Geon-Hong is offline   Reply With Quote

Old   November 24, 2011, 04:29
Default
  #10
Member
 
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 5
robbirobocop is on a distinguished road
Quote:
Originally Posted by Geon-Hong View Post

Regeneration of the grid is only hope? ToT
What program did you use to generate the geometry as well as the grid?
It seems that you would have to regenerate the grid. If you have done it with sHM - it will not take you too long ^^
robbirobocop is offline   Reply With Quote

Old   November 24, 2011, 06:16
Default about grid problems
  #11
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
I've noticed just before that the problems have been occurred far from the wing, not adjacent to the wing.

The problem is that the grid has been generated in structured manner and the grid size along in the downstream was stretched while thin layer of grid for resolving the boundary layer near the wall is maintained.

Now I am considering a hybrid grid arrangement : structured near the wall and unstructured at far field.


Rob / I used gambit to generate the grid. Now I'd like to try Ansys instead. I have no idea about sHM. What is it?
Geon-Hong is offline   Reply With Quote

Old   November 24, 2011, 06:24
Default Fluent
  #12
New Member
 
Geon-Hong Kim
Join Date: Feb 2010
Location: Ulsan, Republic of Korea
Posts: 27
Rep Power: 7
Geon-Hong is on a distinguished road
One more thing that I'd like to mention is that I ran the same case(mesh) with the FLUENT but it provided converged transient solution. At least, FLUENT may provide a transient solution though the mesh have extremely high aspect ratio cells which have order of 1e4 as my case.

From following thread, Mads Reck also referred that

aspect ratios of more than 1000 is by no means insane - we have it in airfoil aerodynamics all the time - and on wind turbine blades.

Aspect ratios of 1e5 or even higher is usual business when you want to have a first cell height of around 1e-6 chordLengths.

results with checkMesh...please comment

I hope to resolve this problem as soon as possible.
Geon-Hong is offline   Reply With Quote

Old   November 24, 2011, 06:39
Default
  #13
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 373
Rep Power: 10
arjun is on a distinguished road
Quote:
Originally Posted by Geon-Hong View Post
One more thing that I'd like to mention is that I ran the same case(mesh) with the FLUENT but it provided converged transient solution. At least, FLUENT may provide a transient solution though the mesh have extremely high aspect ratio cells which have order of 1e4 as my case.

From following thread, Mads Reck also referred that

aspect ratios of more than 1000 is by no means insane - we have it in airfoil aerodynamics all the time - and on wind turbine blades.

Aspect ratios of 1e5 or even higher is usual business when you want to have a first cell height of around 1e-6 chordLengths.

results with checkMesh...please comment

I hope to resolve this problem as soon as possible.

Fluent starccm+ etc apply lots of tricks (trade secrets) to keep solver stable. The main difficulty with high respect ratio is that it makes pressure correction equation very difficult to converge, which could make solver unstable.
OpenFOAM does not apply such tricks so things should be more difficult with it. For this reason you would need good quality meshes with openFOAM.
arjun is offline   Reply With Quote

Old   November 24, 2011, 06:48
Default
  #14
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
Hi,

You have some cells with high nonorthogonality (90 starts to be a high value imo). You should used "limited 0,333" schemes and not "corrected" schemes (snGrad).
I don't know if it would solve your problem, but it should be a start.

Aurelien
Aurelien Thinat 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
the problem of my transient simulation "Floating point exception: Overflow " alloveyou CFX 15 November 22, 2012 12:14
Transient axial rotor/stator convergence issue? Nicola Viscanti CFX 3 March 17, 2010 05:15
Continuity eq convergence problem carno FLUENT 4 February 8, 2008 05:04
convergence problem Trushar Phoenics 5 August 27, 2002 23:40
convergence problem with SIMPLER NURAY KAYAKOL Main CFD Forum 1 February 24, 1999 14:43


All times are GMT -4. The time now is 01:09.