[guilha]

Good afternoon everyone,

I run a flat plate simulation, RANS with rhoCentralFoam, with a 600 probes to compute some boundary layer parameters. It was done in parallel processing, and when I reconstructed the fields...there was no fields. And the probes working were not all, only the first 334 probes defined in the controlDict, that is the folder exists but no sub folders with the starting time and fields.

Summarizing, not all the probes worked (and no warnings was given) and I can not view the fields in paraview. And the program runs without any other problem.

Thanks in advance.

[guilha]

I run other simulation with fewer probes, they did not work at all. Some of them do not have all the time steps.

Does anyone know what is the problem ?

I define the probes in the controlDict in the following way (at the bottom of the file):

functions
(
  probe_number_1
  {
    type probes;
    functionObjectLibs ("libsampling.so");
    region region0;
    probeLocations
    (
      (-0.0100 0.120001 0) 
    );
    fields
    (
      U
    );
  }
)

I must say that in the files where it failed to write the time-steps I can not open the file with gedit.

[wyldckat]

Hi guilha,

I got your private message. I suspect that the problem might be simpler than you expect: you might be running out of disk space. To check this, run:

df -h

And check the entry for "/" or "/home" and check how much it's telling you it has got occupied and how much is free.

On the other hand, if disk space isn't the problem, then I need some more information:

1. Which OpenFOAM version or variant are you using?
2. Which Linux Distribution are you using?
3. What installation instructions have you followed for installing OpenFOAM?
4. How many cells does your mesh have?
5. How much memory does your machine have?
6. How many sub-domains are you using?
7. Are you 100% certain that the mesh has the same geometrical units as the probe locations? In other words, did you open the case in ParaView and placed some "Sphere" sources located at the desired probe locations, to make sure the locations are valid?
8. Did you check the mesh using checkMesh? A complete check is done like this:
   

   checkMesh -allGeometry -allTopology

9. Did you check the contents of the folders "processor*"?
10. What are the time related settings you are using in "controlDict"? It's possible that you missed some minor-looking detail, which might actually influence the time snapshots that are saved.
11. It's also possible that the solver, even though it gave no error message, it might actually have indicated that nothing useful was being calculated. Therefore, can you please provide the last time iteration output from the solver?

I ask all of these questions, because the information you provided isn't enough to diagnose the problem

Best regards,
Bruno

[guilha]

Thank you Bruno,

If the problem is the lack of memory, should not it give this error
http://www.cfd-online.com/Forums/ope...-2-errors.html

- my OpenFOAM version is 2.0.1;
- debian
- I do not know, it might be impossible to know (I am on the university computers)
- 3.1 million cells
- 900 gb but only 100 gb available
- I used 32 nodes and 64 too
- I do not know how to use paraView to view the probes, I found a filter with the option of Probe Location but I could not find out anything, but I suppose the problem is not the location
- the checkMesh (with the two options) said the Mesh is OK but it gave an error

--> FOAM Serious Error : 
    From function IOobject::readHeader(Istream&)
    in file db/IOobject/IOobjectReadHeader.C at line 89
    Reading "/home/guilha/Desktop/resultados/cavidade_LES_130kx24_smagorinsky_perfil_power_law_v3/0.0144/uniform/time" at line 1
    First token could not be read or is not the keyword 'FoamFile'

Check header is of the form:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "0.0144/uniform";
    object      time;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

End

- no I did not, and I erased it to save memory
- my controDict file is (I omitted the probes because I have already put an example)

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     rhoCentralFoam;

startFrom       latestTime;
//startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         0.02;

deltaT          1.0e-07;

writeControl    runTime;

writeInterval   2.0e-04; // É LES...

purgeWrite      0;

writeFormat     ascii;

writePrecision  7;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable false;

adjustTimeStep  no;

functions
(
);

- the last iteration output was

Mean and max Courant Numbers = 0.04979834 0.1448724
Time = 0.02

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal:  Solving for rhoUz, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 1.374598e-06, Final residual = 4.865261e-15, No Iterations 3
smoothSolver:  Solving for Uy, Initial residual = 3.260119e-06, Final residual = 2.374335e-14, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 5.533801e-06, Final residual = 4.280753e-15, No Iterations 3
diagonal:  Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for e, Initial residual = 5.643462e-06, Final residual = 8.838985e-14, No Iterations 3
ExecutionTime = 54098.04 s  ClockTime = 54515 s

End

Finalising parallel run

In the header of my controlDict file it says that the OpenFOAM version is the 2.1.0 but the OpenFOAM's folder name is openfoam201...

When I run simulations I can only run 24 hours, then the computer kills the run. When I rerun, from the previous saved time, a new folder is built in the probe's folder. It was on one of those folders that it did not wrote on every probes. For instance if my signal is from 0-0.01 from 0.008 to 0.009, in some probes there is very few results.

Edit: I can view the results in paraview.

[wyldckat]

Hi Guilha,

Originally Posted by guilha

If the problem is the lack of memory, should not it give this error
http://www.cfd-online.com/Forums/openfoam/78047-2errors.html

Yes, but that might only be true when using a single machine and storing files on that same machine. If it's shared data between more than one machine, there could be some silent problems in the remote file access system. In other words, it pretends that it's writing the file, but actually completely ignores the write requests.

Originally Posted by guilha

- 3.1 million cells

OK, that would be roughly 3 GiB of RAM for running the case.

Originally Posted by guilha

- 900 gb but only 100 gb available

900GB of RAM? That's one powerful machine or cluster!

Originally Posted by guilha

- I used 32 nodes and 64 too

32 and 64 sub-domains... that equates to roughly 96000 and 48000 cells per processor. This could imply that so many divisions could lead to problems with cyclic patches, if there are any present; I say this because cyclic patches use to be a headache to use in parallel running, because the entry "preservePatches" had to be used for making sure the patches were not divided between processors. I can't remember when this was fixed, but I suspect that 2.0.1 did not have this fixed yet.

Originally Posted by guilha

- I do not know how to use paraView to view the probes, I found a filter with the option of Probe Location but I could not find out anything, but I suppose the problem is not the location

Attached are 4 images that tell the story how probe locations can be visualized in ParaView:

1. Run paraFoam and choose to see the outline of the case.
2. You can see the "cube axes", which show the dimensions of the geometry.
3. You can use a "sphere source" (see in the menu "Sources"), for placing a sphere where one of the probes are.
4. In the last image is shown that you can:
   1. Load a CSV file, such as this one:
      

      x, y, z
      0.01, 0.02, 0.005
      0.02, 0.03, 0.005
      0.03, 0.04, 0.005
      0.04, 0.06, 0.005

   2. Apply the filter "Table to points", by indicating which column refers to which axis.
   3. Apply the "Glyphs" filter to the "TableToPoints1" item and configure it accordingly to the image, so that you can see sphere's where the probes are meant to be.

Originally Posted by guilha

- the checkMesh (with the two options) said the Mesh is OK but it gave an error

--> FOAM Serious Error : 
    From function IOobject::readHeader(Istream&)
    in file db/IOobject/IOobjectReadHeader.C at line 89
    Reading "/home/guilha/Desktop/resultados/cavidade_LES_130kx24_smagorinsky_perfil_power_law_v3/0.0144/uniform/time" at line 1

It's indicating that the file "0.0144/uniform/time" is either damaged/corrupted or is a bug, which has already been fixed in 2.0.x or newer versions of OpenFOAM.
But have a look at the contents of the file "0.0144/uniform/time", to check if it's empty or not.

Originally Posted by guilha

- no I did not, and I erased it to save memory

So much for the evidence of the crime

Originally Posted by guilha

- my controDict file is (I omitted the probes because I have already put an example)

rhoCentralFoam is a transient solver... and you turned off the automatic Courant related adjustments for deltaT. Without the checkMesh output, I can't assess if deltaT of "1.0e-07" is enough or not.
Nonetheless, everything seems fine with the settings in "controlDict".

By the way, I strongly suggest that you use the following settings, if you're trying to save disk space:

writeFormat     binary;
writeCompression on;

Originally Posted by guilha

- the last iteration output was
[...]
In the header of my controlDict file it says that the OpenFOAM version is the 2.1.0 but the OpenFOAM's folder name is openfoam201...

The output looks sane... there are no "NaN" values and the Courant number seems low enough. So that shouldn't be the source of the problem.

To check the OpenFOAM version, check the beginning of the output. Actually, we already have gotten the confirmation of the version number, from the error message that checkMesh gave you.

Originally Posted by guilha

When I run simulations I can only run 24 hours, then the computer kills the run. When I rerun, from the previous saved time, a new folder is built in the probe's folder. It was on one of those folders that it did not wrote on every probes. For instance if my signal is from 0-0.01 from 0.008 to 0.009, in some probes there is very few results.

This looks like one or more bugs that have already been fixed in OpenFOAM. I would suggest running for a shorter period of time, for isolating the source of the problem.

As for 24h, there are some job schedulers in clusters that allow requesting for more runtime than the default.

Best regards,
Bruno

[guilha]

Thank you Bruno for your reply,

When I said that the available memory is 900 gb, it is 900 gb to storage data, the RAM is 32 gb. And the memory RAM that this case needs is about 8 gb.

When I used the decomposePar, I used the preservePatch however it gave me random errors again on the first iterations the ones from the printstack thread.

The checkMesh output is:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.0.1-51f1de99a4bc
Exec   : checkMesh -allGeometry -allTopology
Date   : Jan 23 2014
Time   : 13:31:00
Host   : bandido
PID    : 27213
Case   : /home/guilha/Desktop/resultados/cavidade_LES_130kx24_smagorinsky_perfil_power_law_v3
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           3245325
    faces:            9431000
    internal faces:   9128872
    cells:            3093312
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     3093312
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                   Bounding box
    entrada             5280     5525     ok (non-closed singly connected)   (-0.05 0.12 -0.06) (-0.05 0.22 0.06)
    topo                11424    11925    ok (non-closed singly connected)   (-0.05 0.22 -0.06) (0.25 0.22 0.06)
    saida               5280     5525     ok (non-closed singly connected)   (0.25 0.12 -0.06) (0.25 0.22 0.06)
    parede              22368    23325    ok (non-closed singly connected)   (-0.05 0 -0.06) (0.25 0.12 0.06)
    tras                128888   129813   ok (non-closed singly connected)   (-0.05 0 -0.06) (0.25 0.22 -0.06)
    frente              128888   129813   ok (non-closed singly connected)   (-0.05 0 0.06) (0.25 0.22 0.06)

Checking geometry...
    Overall domain bounding box (-0.05 0 -0.06) (0.25 0.22 0.06)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (3.435074e-15 6.089719e-15 2.451804e-14) OK.
    Max cell openness = 2.149904e-16 OK.
    Max aspect ratio = 12.2 OK.
    Minumum face area = 1.70765e-07. Maximum face area = 5.854043e-06.  Face area magnitudes OK.
    Min volume = 8.53825e-10. Max volume = 2.927022e-09.  Total volume = 0.00432.  Cell volumes OK.
    Mesh non-orthogonality Max: 0 average: 0
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.927997e-06 OK.
    Face tets OK.
    Min/max edge length = 0.000409836 0.005 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : average = 1  min = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 0.03420856 average: 0.588144
    Cell determinant check OK.
    Concave cell check OK.

Mesh OK.

--> FOAM Serious Error : 
    From function IOobject::readHeader(Istream&)
    in file db/IOobject/IOobjectReadHeader.C at line 89
    Reading "/home/guilha/Desktop/resultados/cavidade_LES_130kx24_smagorinsky_perfil_power_law_v3/0.0144/uniform/time" at line 1
    First token could not be read or is not the keyword 'FoamFile'

Check header is of the form:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "0.0144/uniform";
    object      time;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

End

And the files from that folder seem ok.

The probes, I could not do csv file because there is too many probes but they are definitely in the domain. And I say it again that it only did not save some iterations from one time file.

Off-topic 1 I had this output in the checkMesh (other case, RANS k-omega)

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.0.1-51f1de99a4bc
Exec   : checkMesh -allGeometry -allTopology
Date   : Jan 23 2014
Time   : 14:21:31
Host   : bandido
PID    : 27432
Case   : /home/guilha/Desktop/resultados/cavidade_RANS_32k_pontos_k_omega_SST
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           63210
    internal points:  0
    edges:            157095
    internal edges:   30679
    internal edges using one boundary point:   0
    internal edges using two boundary points:  30679
    faces:            125027
    internal faces:   61819
    cells:            31141
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     31141
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
  <<Writing 6 cells with with two non-boundary faces to set twoInternalFacesCells
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                   Bounding box
    entrada             114      230      ok (non-closed singly connected)   (-0.05 0.12 -0.06) (-0.05 0.22 0.06)
    topo                216      434      ok (non-closed singly connected)   (-0.05 0.22 -0.06) (0.25 0.22 0.06)
    saida               114      230      ok (non-closed singly connected)   (0.25 0.12 -0.06) (0.25 0.22 0.06)
    parede_longitudinal 167      338      ok (non-closed singly connected)   (-0.05 0.12 -0.06) (0.25 0.12 0.06)
    parede_sem_funcao_de_parede315      632      ok (non-closed singly connected)   (0 0 -0.06) (0.05 0.12 0.06)
    trasEfrente         62282    63210    ok (non-closed singly connected)   (-0.05 0 -0.06) (0.25 0.22 0.06)

Checking geometry...
    Overall domain bounding box (-0.05 0 -0.06) (0.25 0.22 0.06)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (-5.6637258e-17 -4.5615823e-16 -3.0267009e-15) OK.
    Max cell openness = 2.2156954e-16 OK.
    Max aspect ratio = 361.70727 OK.
    Minumum face area = 4.4305555e-09. Maximum face area = 0.00027692309.  Face area magnitudes OK.
    Min volume = 5.3166666e-10. Max volume = 2.6373629e-07.  Total volume = 0.00432.  Cell volumes OK.
    Mesh non-orthogonality Max: 0.12530119 average: 0.0010267398
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.00093247095 OK.
    Face tets OK.
    Min/max edge length = 6.38e-06 0.12 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : average = 1  min = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 0.000120951 average: 3.5305081
 ***Cells with small determinant found, number of cells: 5
  <<Writing 5 under-determined cells to set underdeterminedCells
    Concave cell check OK.

Failed 1 mesh checks.

End

It only runs for 6 seconds then it gives the printstack error, this is because of the mesh ? I have put the first cell very close to the wall.

Off-topic 2 when I use paraview to view the colour plots I have always the average on the cells, I do not have the option to select the color by interpolation. Is this why I can not plot the streamlines nor isosurface and contour plots ?

[wyldckat]

Hi guilha,

Originally Posted by guilha

When I said that the available memory is 900 gb, it is 900 gb to storage data, the RAM is 32 gb. And the memory RAM that this case needs is about 8 gb.

Ah, OK.

Originally Posted by guilha

When I used the decomposePar, I used the preservePatch however it gave me random errors again on the first iterations the ones from the printstack thread.

Mmm... I think you mean this post: http://www.cfd-online.com/Forums/ope...tml#post456884 post #35
I'm starting to feel that you should try and upgrade to the latest OpenFOAM version, because I think this is a bug that has been fixed a long time ago.

Originally Posted by guilha

The checkMesh output is:

[...]And the files from that folder seem ok.

The mesh does seem to be perfectly OK.
What does the file "0.0144/uniform/time" contain?
Again I suspect this is another bug that has already been fixed.

Originally Posted by guilha

The probes, I could not do csv file because there is too many probes but they are definitely in the domain. And I say it again that it only did not save some iterations from one time file.

Well, a few of random points from the list would have been enough.
The problem is only when you continued the simulation? Then I suspect that it's a bug that has already been fixed in the latest versions. Keep in mind that you are using 2.0.1 and the latest is 2.2.2.

Originally Posted by guilha

Off-topic 1 I had this output in the checkMesh (other case, RANS k-omega)

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.0.1-51f1de99a4bc
Exec   : checkMesh -allGeometry -allTopology
Date   : Jan 23 2014
Time   : 14:21:31
Host   : bandido
PID    : 27432
Case   : /home/guilha/Desktop/resultados/cavidade_RANS_32k_pontos_k_omega_SST
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           63210
    internal points:  0
    edges:            157095
    internal edges:   30679
    internal edges using one boundary point:   0
    internal edges using two boundary points:  30679
    faces:            125027
    internal faces:   61819
    cells:            31141
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     31141
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
  <<Writing 6 cells with with two non-boundary faces to set twoInternalFacesCells
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                   Bounding box
    entrada             114      230      ok (non-closed singly connected)   (-0.05 0.12 -0.06) (-0.05 0.22 0.06)
    topo                216      434      ok (non-closed singly connected)   (-0.05 0.22 -0.06) (0.25 0.22 0.06)
    saida               114      230      ok (non-closed singly connected)   (0.25 0.12 -0.06) (0.25 0.22 0.06)
    parede_longitudinal 167      338      ok (non-closed singly connected)   (-0.05 0.12 -0.06) (0.25 0.12 0.06)
    parede_sem_funcao_de_parede315      632      ok (non-closed singly connected)   (0 0 -0.06) (0.05 0.12 0.06)
    trasEfrente         62282    63210    ok (non-closed singly connected)   (-0.05 0 -0.06) (0.25 0.22 0.06)

Checking geometry...
    Overall domain bounding box (-0.05 0 -0.06) (0.25 0.22 0.06)
    Mesh (non-empty, non-wedge) directions (1 1 0)
    Mesh (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (-5.6637258e-17 -4.5615823e-16 -3.0267009e-15) OK.
    Max cell openness = 2.2156954e-16 OK.
    Max aspect ratio = 361.70727 OK.
    Minumum face area = 4.4305555e-09. Maximum face area = 0.00027692309.  Face area magnitudes OK.
    Min volume = 5.3166666e-10. Max volume = 2.6373629e-07.  Total volume = 0.00432.  Cell volumes OK.
    Mesh non-orthogonality Max: 0.12530119 average: 0.0010267398
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.00093247095 OK.
    Face tets OK.
    Min/max edge length = 6.38e-06 0.12 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : average = 1  min = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 0.000120951 average: 3.5305081
 ***Cells with small determinant found, number of cells: 5
  <<Writing 5 under-determined cells to set underdeterminedCells
    Concave cell check OK.

Failed 1 mesh checks.

End

It only runs for 6 seconds then it gives the printstack error, this is because of the mesh ? I have put the first cell very close to the wall.

checkMesh is telling you that have a mesh that looks like a 2D case, but it has one or more faces/patches that are on one or both sides of the empty direction.

Originally Posted by guilha

Off-topic 2 when I use paraview to view the colour plots I have always the average on the cells, I do not have the option to select the color by interpolation. Is this why I can not plot the streamlines nor isosurface and contour plots ?

Strange... what is the exact command or commands you use to open in ParaView?
And which file extension? ".OpenFOAM", ".foam" or ".VTK"?

Best regards,
Bruno

[guilha]

Hello Bruno, thanks for your replies.

I think the same about the OpenFOAM versions, but that does not depend on me. Does newer versions accept the same files ?

About the off-topics, the 1st it is the same mesh (blocks and boundaries) of another case I ran (RANS k-epsilon, but I put the first cell farther the k-omega) so it seems strange to me that it is badly built.

The second, I execute the command foamToEnsight then I simply open ParaView with ./paraview, the file extension is .case

[wyldckat]

Hi guilha,

Originally Posted by guilha

I think the same about the OpenFOAM versions, but that does not depend on me. Does newer versions accept the same files ?

Yes and no. Usually minor adjustments are needed to the case set-up, in order to maintain the same use. In other words: it's mostly compatible.
You can at least try building/using OpenFOAM 2.0.x - http://www.openfoam.org/download/git.php but replace 2.2.x for 2.0.x - which has several bug fixes in the 2.0 series and should be directly compatible with 2.0.1.

The other possibility is to talk to your supervisor and/or cluster administrator and up the time constraint for your runs to 48h or 72h. It's LES, therefore 24h is waaay too little time to solve anything.

Originally Posted by guilha

About the off-topics, the 1st it is the same mesh (blocks and boundaries) of another case I ran (RANS k-epsilon, but I put the first cell farther the k-omega) so it seems strange to me that it is badly built.

What exactly are you referring to when you say: «but I put the first cell farther the k-omega»
In other words, what was the change you made in "blockMeshDict"?

Originally Posted by guilha

The second, I execute the command foamToEnsight then I simply open ParaView with ./paraview, the file extension is .case

Ensight format? Which ParaView version are you using?
If you are using 3.10.1 or 3.12.0, run:

touch case.foam
paraview

and choose to open the file "case.foam". You'll get a much better reader interface.

Best regards,
Bruno

[guilha]

The meshes only have one difference that is on the walls.
My first point of the block which contains the wall in one case is closer to the wall than the other.

Something like this:
.......................................
______________________
\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\


.......................................


______________________
\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\

This is to respect the y+.

The paraview version I have is the 3.14.1 64 bit.

[wyldckat]

Originally Posted by guilha

The meshes only have one difference that is on the walls.
My first point of the block which contains the wall in one case is closer to the wall than the other.

Something like this:
.......................................
______________________
\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\


.......................................


______________________
\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\

This is to respect the y+.

You only changed 1 point? If I'm picturing your case correctly in my mind, you need to move at least 4 points, which represent a rectangle/square! Or at the very least, change 2 points, one on each side of the empty patches.

Originally Posted by guilha

The paraview version I have is the 3.14.1 64 bit.

Even better! Follow the steps I mentioned and you should get a much better user interface.

[guilha]

Sorry, of course it was not only one point, what I meant was that I only changed one thing which was the position of the points just next to the wall. I did not know I had my mesh with a bad topology, I only realised it now

However, I found out that increasing the distance it does not give any problem in the determinants.

[skmaperu]

hello ,

i am facing similar problem
i have check the storage space. its fine

the problem i dectected is 0 directory missing in processor folder.
and while decomposing . i have seen a message stating

First token could not be read or is not the keyword 'FoamFile'


thanks in advance

manikanth

[wyldckat]

Originally Posted by skmaperu

and while decomposing . i have seen a message stating

First token could not be read or is not the keyword 'FoamFile'

Quick answer: If that error message is given while running decomposePar, then we need more details. What is the complete message that decomposePar gives you?